Corporate Address 
Livermore Software Technology Corporation 
P.  O.  Box 712 
Livermore, California 94551-0712 
Support Addresses 
LSTC 
7374 Las Positas Road 
Livermore, California 94551 
Tel:  925-449-2500  ♦  Fax:  925-449-2507 
Email:  sales@lstc.com 
Website:  www.lstc.com 
Disclaimer 
LSTC 
1740 West Big Beaver Road 
Suite 100 
Troy, Michigan  48084 
Tel:  248-649-4728  ♦  Fax:  248-649-6328 
Copyright  ©  1992-2017  Livermore  Software  Technology  Corporation.    All  Rights 
Reserved. 
LS-DYNA®, LS-OPT® and LS-PrePost® are registered trademarks of Livermore Software 
Technology Corporation in the United States.  All other trademarks, product names and 
brand names belong to their respective owners. 
LSTC  reserves  the  right  to  modify  the  material  contained  within  this  manual  without 
prior  notice. 
The  information  and  examples  included  herein  are  for  illustrative  purposes  only  and 
are  not  intended  to  be  exhaustive  or  all-inclusive.    LSTC  assumes  no  liability  or 
responsibility whatsoever for any direct of indirect damages or inaccuracies of any type 
or nature that could be deemed to have resulted from the use of this manual. 
Any  reproduction,  in  whole  or  in  part,  of  this  manual  is  prohibited  without  the  prior 
written approval of LSTC.  All requests to reproduce the contents hereof should be sent 
to sales@lstc.com. 
⎯⎯⎯⎯⎯⎯⎯⎯⎯⎯⎯⎯⎯⎯⎯⎯⎯⎯⎯ 
AES Licensing Terms 
Copyright © 2001, Dr Brian Gladman < brg@gladman.uk.net>, Worcester, UK.  All rights reserved. 
The free distribution and use of this software in both source and binary form is allowed (with or without 
changes) provided that: 
1.distributions of this source code include the above copyright notice, this list of conditions and the 
following disclaimer; 
2.distributions  in  binary  form  include  the  above  copyright  notice,  this  list  of  conditions  and  the 
following disclaimer in the documentation and/or other associated materials; 
3.he  copyright  holder's  name  is  not  used  to  endorse  products  built  using  this  software  without 
specific written permission.  
DISCLAIMER 
This  software  is  provided  'as  is'  with  no  explicit  or  implied  warranties  in  respect  of  any  properties, 
including, but not limited to, correctness and fitness for purpose.
This file contains the code for implementing the key schedule for AES (Rijndael) for block and key sizes 
of 16, 24, and 32 bytes.
When  defining  an  equation  of  state,  the  type  of  equation  of  state  is  specified  by  a 
corresponding  3-digit  number  in  the  command  name,  e.g.,  *EOS_004,  or  equivalently, 
by  it’s  more  descriptive  designation,  e.g.,  *EOS_GRUNEISEN.    The  equations  of  state 
can be used with a subset of the materials that are available for solid elements; see the 
MATERIAL  MODEL  REFERENCE  TABLES  in  the  beginning  of  the  *MAT  section  of 
this Manual.   *EOS_015 is linked to the type 2 thick shell element and can be  used to 
model engine gaskets. 
The meaning associated with particular extra history variables for a subset of material 
models and equations of state are  tabulated at http://www.dynasupport.com/howtos-
/material/history-variables.    The  first  three  extra  history  variables  when  using  an 
equation of state are (1) internal energy, (2) pressure due to bulk viscosity, and (3) the 
element volume from the previous time step. 
TYPE 1: 
*EOS_LINEAR_POLYNOMIAL 
TYPE 2: 
*EOS_JWL 
TYPE 3: 
*EOS_SACK_TUESDAY 
TYPE 4: 
*EOS_GRUNEISEN 
TYPE 5: 
*EOS_RATIO_OF_POLYNOMIALS 
TYPE 6: 
*EOS_LINEAR_POLYNOMIAL_WITH_ENERGY_LEAK 
TYPE 7: 
*EOS_IGNITION_AND_GROWTH_OF_REACTION_IN_HE 
TYPE 8: 
*EOS_TABULATED_COMPACTION 
TYPE 9: 
*EOS_TABULATED 
TYPE 10: 
*EOS_PROPELLANT_DEFLAGRATION 
TYPE 11: 
*EOS_TENSOR_PORE_COLLAPSE 
TYPE 12: 
*EOS_IDEAL_GAS 
TYPE 14: 
*EOS_JWLB 
TYPE 15: 
*EOS_GASKET
*EOS_MIE_GRUNEISEN  
TYPE 19: 
*EOS_MURNAGHAN 
TYPE 21-30: 
*EOS_USER_DEFINED 
An additional option TITLE may be appended to all the *EOS keywords.  If this option 
is used then an additional line is read for each section in 80a format which can be used 
to describe the equation of state.  At present LS-DYNA does not make use of the title.  
Inclusion of title simply gives greater clarity to input decks. 
Definitions and Conventions 
In  order  to  prescribe  the  boundary  and/or  initial  thermodynamic  condition,  manual 
computations  are  often  necessary.    Conventions  or  definitions  must  be  established  to 
simplify this process.  Some basic variables are defined in the following.  Since many of 
these variables have already been denoted by different symbols, the notations used here 
are  unique  in  this  section  only!    They  are  presented  to  only  clarify  their  usage.    A 
corresponding SI unit set is also presented as an example. 
First consider a few volumetric parameters since they are a measure of compression (or 
expansion). 
Volume: 
Mass: 
𝑉 ≈ (m3) 
𝑀 ≈ (Kg) 
Current specific volume (per mass): 
Reference specific volume: 
Relative volume: 
𝜐 =
=
≈ (
𝑚3
Kg
) 
𝜐0 =
𝑉0
=
𝜌0
≈ (
𝑚3
Kg
) 
𝜐𝑟 =
𝑉0
=
)
(𝑉 𝑀⁄
(𝑉0 𝑀⁄
)
=
𝜐0
=
𝜌0
Current normalized volume increment: 
𝑑𝜐
=
𝜐 − 𝜐0
= 1 −
𝜐𝑟
= 1 −
𝜌0
𝜇 =
𝜐𝑟
− 1 =
𝜐0 − 𝜐
= −
𝑑𝜐
=
𝜌0
− 1 
Sometimes another volumetric parameter is used: 
𝜌0
𝜐0
𝜂 =
=
Thus, the relation between 𝜇 and 𝜂  is, 
𝜇 =
𝜐0 − 𝜐
= 𝜂 − 1 
The following table summarizes these volumetric parameters. 
VARIABLES 
COMPRESSION 
NO LOAD 
EXPANSION 
𝜐𝑟 =
𝜐0
=
𝜌0
𝜂 =
𝜐𝑟
=
𝜐0
=
𝜌0
𝜇 =
𝜐𝑟
− 1 = 𝜂 − 1 
< 1 
> 1 
> 0 
V0 – Initial Relative Volume 
1 
1 
0 
> 1 
< 1 
< 0 
There are 3 definitions of density that must be distinguished from each other: 
𝜌0 = 𝜌ref 
= Density at nominal reference
⁄
state, usually non-stress or non-deformed state. 
𝜌∣𝑡=0 = Density at time 0 
𝜌  = Current density 
Recalling the current relative volume 
𝜐𝑟 =
𝜌0
=
𝜐0
, 
at time = 0 the relative volume is 
𝜐𝑟0 = 𝜐𝑟|𝑡=0 =
𝜌0
𝜌∣𝑡=0
=
𝜐|𝑡=0
𝜐0
. 
Generally, the V0 input parameter in an *EOS card refers to this 𝜐𝑟0.  𝜌0 is generally the 
density defined in the *MAT card.  Hence, if a material is mechanically compressed at
(𝜐0 ≠ 𝑉0). 
The “reference” state is a unique state with respect to which the material stress tensor is 
computed.    Therefore  𝜐0  is  very  critical  in  computing  the  pressure  level  in  a  material.  
Incorrect  choice  of  𝜐0  would  lead  to  incorrect  pressure  computed.    In  general,  𝜐0  is 
chosen  such  that  at  zero  compression  or  expansion,  the  material  should  be  in 
equilibrium with its ambient surrounding.  In many of the equations shown in the EOS 
section, 𝜇 is frequently used as a measure of compression (or expansion).  However, the 
users must clearly distinguish between 𝜇 and 𝜐𝑟0. 
E0 – Internal Energy 
Internal  energy  represents 
component) of a system.  One definition for internal energy is 
thermal  energy  state 
the 
(temperature  dependent 
𝐸 = 𝑀𝐶𝑣𝑇 ≈ (Joule) 
Note that the capital “𝐸” here is the absolute internal energy.  It is not the same as that 
used  in  the  subsequent  *EOS  keyword  input,  or  some  equations  shown  for  each  *EOS 
card.  This internal energy is often defined with respect to a mass or volume unit. 
Internal energy per unit mass (also called specific internal energy): 
𝑒 =
= 𝐶𝑉𝑇 ≈ (
Joule
Kg
) 
Internal energy per unit current volume:  
𝑒𝑉 =
𝐶𝑉𝑇 = 𝜌𝐶𝑉𝑇 =
𝐶𝑉𝑇
≈ (
Joule
m3 =
m2) 
Internal energy per unit reference volume: 
𝑒𝑉0 =
𝑉0
𝐶𝑣𝑇 = 𝜌0𝐶𝑣𝑇 =
𝐶𝑣𝑇
𝜐0
≈ (
Joule
m3 =
m2) 
𝑒𝑉0  typically  refers  to  the  capital  “E”  shown  in  some  equations  under  this  “EOS” 
section.  Hence the initial “internal energy per unit reference volume”, E0, a keyword input 
parameter in the *EOS section can be computed from 
To convert from 𝑒𝑉0 to 𝑒𝑉, simply divide 𝑒𝑉0 by 𝜐𝑟 
𝑒𝑉0∣
𝑡=0
= 𝜌0𝐶𝑉𝑇|𝑡=0 
𝑒𝑉 = 𝜌𝐶𝑉𝑇 = [𝜌0𝐶𝑉𝑇]
𝜌0
=
𝑒𝑉0
𝜐𝑟
A  thermodynamic  state  of  a  homogeneous  material,  not  undergoing  any  chemical 
reactions  or  phase  changes,  may  be  defined  by  two  state  variables.    This  relation  is 
generally  called  an  equation  of  state.    For  example,  a  few  possible  forms  relating 
pressure to two other state variables are 
𝑃 = 𝑃(𝜌, 𝑇) = 𝑃(𝜐, 𝑒) = 𝑃(𝜐𝑟, 𝑒𝑉) = 𝑃(𝜇, 𝑒𝑉0) 
The last equation form is frequently used to compute pressure.  The EOS for solid phase 
materials is sometimes partitioned into 2 terms, a cold pressure and a thermal pressure  
𝑃 = 𝑃𝑐(𝜇) + 𝑃𝑇(𝜇, 𝑒𝑉0) 
𝑃𝑐(𝜇)  is  the  cold  pressure  hypothetically  evaluated  along  a  0-degree-Kelvin  isotherm.  
This  is  sometimes  called  a  0-K  pressure-volume  relation  or  cold  compression  curve.  
𝑃𝑇(𝜇, 𝑒𝑉0)  is  the  thermal  pressure  component  that  depends  on  both  volumetric 
compression and thermal state of the material.  
Different  forms  of  the  EOS  describe  different  types  of  materials  and  how  their 
volumetric compression (or expansion) behaviors.  The coefficients for each EOS model 
come  from  data-fitting,  phenomenological  descriptions,  or  derivations  based  on 
classical thermodynamics, etc. 
Linear Compression 
In low pressure processes, pressure is not significantly affected by temperature.  When 
volumetric  compression  is  within  an  elastic  linear  deformation  range,  a  linear  bulk 
modulus  may  be  used  to  relate  volume  changes  to  pressure  changes.    Recalling  the 
definition of an isotropic bulk modulus is [Fung 1965], 
This may be rewritten as 
Δ𝜐
= −
. 
𝑃 = 𝐾 [−
Δ𝜐
] = 𝐾𝜇. 
The bulk modulus, 𝐾, thus is equivalent to 𝐶1 in *EOS_LINEAR_POLYNOMIAL when 
all other coefficients are zero.  This is a simplest form of an EOS.  To initialize a pressure 
for such a material, only 𝜐𝑟0 must be defined. 
Initial Conditions 
In general, a thermodynamic state must be defined by two state variables.  The need to 
specify  𝜐𝑟0  and/or  𝑒𝑉0∣
  depends  on  the  form  of  the  EOS  chosen.    The  user  should 
review the equation term-by-term to establish what parameters to be initialized. 
𝑡=0
or  𝜐𝑟0.    Consider  two  possibilities  (1)  𝑇|𝑡=0  is  defined  or 
assumption  on  either  𝑒𝑉0∣
assumed from which 𝑒𝑉0∣
 may be computed, or (2) 𝜌∣𝑡=0 is defined or assumed from 
𝑡=0
which 𝜐𝑟0 may be obtained. 
𝑡=0
When to Use EOS 
For  small  strains  considerations,  a  total  stress  tensor  may  be  partitioned  into  a 
deviatoric stress component and a mechanical pressure. 
𝜎𝑖𝑗 = 𝜎𝑖𝑗
′ +
𝜎𝑘𝑘
𝛿𝑖𝑗 = 𝜎𝑖𝑗
′ − 𝑃𝛿𝑖𝑗 
𝑃 = −
𝜎𝑘𝑘
The pressure component may be written from the diagonal stress components. 
Note that 
𝜎𝑘𝑘
3 =
[𝜎11+𝜎22+𝜎33]
 is positive in tension while P is positive in compression.   
Similarly, the total strain tensor may be partitioned into a deviatoric strain component 
(volume-preserving deformation) and a volumetric deformation. 
𝜀𝑘𝑘
𝜀𝑘𝑘
3   is  called  the  mean  normal  strain,  and  𝜀𝑘𝑘  is  called  the  dilatation  or  volume 
𝜀𝑖𝑗 = 𝜀𝑖𝑗
′ +
𝛿𝑖𝑗 
where 
strain (change in volume per unit initial volume) 
𝜀𝑘𝑘 =
𝑉 − 𝑉0
𝑉0
′ )  as  a 
Roughly  speaking,  a  typical  convention  may  refer  to  the  relation  𝜎𝑖𝑗
“constitutive  equation”,  and  𝑃 = 𝑓 (𝜇, 𝑒𝑉0)  as  an  EOS.    The  use  of  an  EOS  may  be 
omitted only when volumetric deformation is very small, and |𝑃| A ∣𝜎𝑖𝑗
′ = 𝑓 (𝜀𝑖𝑗
′ ∣. 
A Note About Contact When Using an Equation of State 
When  a  part  includes  an  equation  of  state,  it  is  important  that  the  initial  geometry  of 
that part not be perturbed by the contact algorithm.  Such perturbation can arise due to 
initial  penetrations  in  the  contact  surfaces  but  can  usually  be  avoided  by  setting  the 
variable IGNORE to 1 or 2 in the *CONTACT input or by using a segment based contact 
(SOFT = 2).
This is Equation of state Form 1. 
*EOS_LINEAR_POLYNOMIAL 
Purpose: 
thermodynamic state of the material by defining E0 and V0 below. 
  Define  coefficients  for  a  linear  polynomial  EOS,  and  initialize  the 
  Card 1 
1 
Variable 
EOSID 
Type 
A8 
  Card 2 
Variable 
1 
E0 
Type 
F 
  VARIABLE   
EOSID 
C0 
C1 
⋮ 
C6 
E0 
V0 
3 
C1 
F 
3 
4 
C2 
F 
4 
5 
C3 
F 
5 
6 
C 4 
F 
6 
7 
C5 
F 
7 
8 
C6 
F 
8 
2 
C0 
F 
2 
V0 
F 
DESCRIPTION
Equation  of  state  ID,  a  unique  number  or  label  not  exceeding  8
characters must be specified. 
The 0th polynomial equation coefficient. 
The 1st polynomial equation coefficient (when used by itself, this
is the elastic bulk modulus, i.e.  it cannot be used for deformation
that is beyond the elastic regime). 
⋮
The 6th polynomial equation coefficient. 
Initial  internal  energy  per  unit  reference  volume  . 
Initial relative volume .
*EOS 
1.  The  linear  polynomial  equation  of  state  is  linear  in  internal  energy.    The 
pressure is given by: 
𝑃 = 𝐶0 + 𝐶1𝜇 + 𝐶2𝜇2 + 𝐶3𝜇3 + (𝐶4 + 𝐶5𝜇 + 𝐶6𝜇2)𝐸. 
𝐶2𝜇2  
 is the ratio 
where terms
of  current  density  to  reference  density.    𝜌  is  a  nominal  or  reference  density 
defined in the *MAT_NULL card.   
are set to zero if 𝜇 < 0, 𝜇 =
− 1, and
and
𝐶6𝜇2
𝜌0
𝜌0
The  linear  polynomial  equation  of  state  may  be  used  to  model  gas  with  the 
gamma law equation of state.  This may be achieved by setting: 
𝐶0 = 𝐶1 = 𝐶2 = 𝐶3 = 𝐶6 = 0 
and 
where  
𝐶4 = 𝐶5 = 𝛾 − 1 
𝛾 =
𝐶𝑝
𝐶𝑣
is the ratio of specific heats.  Pressure for a perfect gas is then given by: 
𝑝 = (𝛾 − 1)
𝜌0
𝐸 
E has the unit of pressure (where 𝜌 and 𝜌) 
2.  When 𝐶0 = 𝐶1 = 𝐶2 = 𝐶3 = 𝐶6 = 0, it does not necessarily mean that the initial 
pressure  is  zero,  𝑃0    ≠ 𝐶0!    The  initial  pressure  depends  the  values  of  all  the 
coefficients and on 𝜇∣𝑡=0 and 𝐸∣𝑡=0.  The pressure in a material is computed from 
the whole equation above, 𝑃 = 𝑃(μ, 𝐸).  It is always  preferable to initialize the 
initial condition based on 𝜇∣𝑡=0 and 𝐸∣𝑡=0.  The use of 𝐶0 = 𝐶1 = 𝐶2 = 𝐶3 = 𝐶6 =
0  must  be  done  with  caution  as  it  may  change  the  form  and  behavior  of  the 
material.    The  safest  way  is  to  use  the  whole  EOS  equation  to  manually  check 
for the pressure value.  For example, for ideal gas, for ideal gas, only 𝐶4 and 𝐶5 
are  nonzero,  𝐶4 = 𝐶5 = 𝛾 − 1  and  all  other  coefficients  𝐶0 = 𝐶1 = 𝐶2 = 𝐶3 =
𝐶6 = 0 to satisfy the perfect gas equation form.  
3.  V0 and E0 defined in this card must be the same as the time-zero ordinates for 
the  2  load  curves  defined  in  the  *BOUNDARY_AMBIENT_EOS  card,  if  it  is 
used.  This is so that they would both consistently define the same initial state 
for a material.
This is Equation of state Form 2. 
Available options are: 
<BLANK> 
AFTERBURN 
*EOS_JWL 
  Card 1 
1 
Variable 
EOSID 
Type 
A8 
2 
A 
F 
3 
B 
F 
4 
R1 
F 
5 
R2 
F 
6 
OMEG 
F 
7 
E0 
F 
8 
VO 
F 
Afterburn card. Additional card for afterburn option with OPT = 1 or 2. 
  Card 2 
1 
Variable 
OPT 
Type 
F 
2 
QT 
F 
3 
T1 
F 
4 
T2 
F 
5 
6 
7 
8 
Afterburn card. Additional card for afterburn option with OPT = 3. 
  Card 2 
1 
Variable 
OPT 
Type 
F 
2 
Q0 
F 
3 
QA 
F 
4 
QM 
5 
6 
7 
8 
QN 
CONM 
CONL 
CONT 
F 
F 
F 
1. 
F 
1. 
F 
1. 
Default 
none 
none 
none 
0.5 
1/6 
  VARIABLE   
EOSID 
1-18 (EOS) 
DESCRIPTION
Equation  of  state  ID,  a  unique  number  or  label  not  exceeding  8
DESCRIPTION
*EOS 
A 
B 
R1 
R2 
𝐴, See equation in Remarks. 
𝐵, See equation in Remarks. 
𝑅1, See equation in Remarks. 
𝑅2, See equation in Remarks. 
OMEG 
𝜔, See equation in Remarks. 
E0 
V0 
OPT 
QT 
T1 
T2 
Q0 
QA 
QM 
QN 
Detonation  energy  per  unit  volume  and  initial  value  for 𝐸.    See 
equation in Remarks. 
Initial  relative  volume,  which  gives  the  initial  value  for  𝑉.    See 
equation in Remarks. 
Afterburn option 
    EQ.0.0: No afterburn energy (Standard EOS_JWL) 
    EQ.1.0: Constant rate of afterburn energy added between times 
                  T1 and T2 
    EQ.2.0: Linearly-increasing rate of afterburn energy added  
                  between times T1 and T2 
    EQ.3.0: Miller’s extension for afterburn energy 
Afterburn  energy  per  unit  volume 
(OPT = 1,2) 
for  simple  afterburn
Start time of energy addition for simple afterburn  
End time of energy addition for simple afterburn 
Afterburn  energy  per  unit  volume  for  Miller’s  extension
(OPT = 3) 
Energy release constant 𝑎 for Miller’s extension 
Energy release exponent 𝑚 for Miller’s extension 
Pressure exponent 𝑛 for Miller’s extension
CONM 
CONL 
CONT 
Remarks: 
*EOS_JWL 
DESCRIPTION
GT.0.0:  Mass  conversion  factor  from  model  units  to  calibration
units 
              for Miller’s extension 
LT.0.0:  Use  predefined  factors  to  convert  model  units  to
published     
             calibration units of g, cm, µs.  Choices for model units are:
              EQ.-1.0: g, mm, ms  
              EQ.-2.0: g, cm, ms  
              EQ.-3.0: kg, m, s 
              EQ.-4.0: kg, mm, ms 
              EQ.-5.0: metric ton, mm, s 
              EQ.-6.0: lbf-s2/in, in, s 
              EQ.-7.0: slug, ft, s 
CONM.GT.0.0: Length conversion factor from model units to  
                           calibration units for Miller’s extension 
CONM.LT.0.0: Ignored 
CONM.GT.0.0: Time conversion factor from model units to  
                           calibration units for Miller’s extension 
CONM.LT.0.0: Ignored 
The JWL equation of state defines the pressure as 
𝑝 = 𝐴 (1 −
𝑅1𝑉
) 𝑒−𝑅1𝑉 + 𝐵 (1 −
𝑅2𝑉
) 𝑒−𝑅2𝑉 +
𝜔𝐸
, 
and is usually used for detonation products of high explosives. 
A,  B,  and    E0  have  units  of  pressure.    R1,  R2,  OMEG,  and  V0  are dimensionless.    It  is 
recommended  that  a  unit  system  of  gram,  centimeter,  microsecond  be  used  when  a 
model includes high explosive(s).   In this consistent unit system, pressure is in Mbar.    
When  this  equation  of  state  is  used  with  *MAT_HIGH_EXPLOSIVE_BURN  in  which 
the variable BETA is set to 0 or 2, the absolute value of the history variable labeled as 
“effective  plastic  strain”  is  the  explosive  lighting  time.    This  lighting  time  takes  into 
account shadowing if invoked .   
There are four additional history variables for the JWL equation of state.  Those history 
variables  are  internal  energy,  bulk  viscosity  in  units  of  pressure,  volume,  and  burn
fraction,  respectively.    To  output  the  history  variables,  set  the  variable  NEIPH  in 
*DATABASE_EXTENT_BINARY.  
The AFTERBURN option allows the addition of afterburn energy 𝑄 to the calculation of 
pressure  by  replacing  𝐸  in  the  above  equation  with  (𝐸 + 𝑄),  i.e.    the  last  term  on  the 
right-hand side becomes 
𝜔(𝐸 + 𝑄)
The simple afterburn option adds the energy at a constant rate (OPT = 1) or a linearly-
increasing rate (OPT = 2) between times T1 and T2 such that the total energy added per 
unit volume at time T2 is the specified energy QT.  
For  the  Miller’s  extension  model  (OPT = 3),  the  afterburn  energy  is  added  via  a  time-
dependent growth term 
𝑑𝜆
𝑑𝑡
= 𝑎(1 − 𝜆)𝑚𝑝𝑛,         𝑄 = 𝜆𝑄0 
Here,  𝑚,  𝑛,  and  𝜆  are  dimensionless,  with  𝜆  a  positive  fraction  less  than  1.0.    The 
parameter  𝑎  has  units  consistent  with  this  growth  equation,  and  𝑄0  has  units  of 
pressure. 
The values for 𝑄0, 𝑎, 𝑚, 𝑛 published by Miller and Guirguis (1993) are calibrated in the 
units  of  g,  cm,  µs,  with  the  consistent  pressure  unit  of  Mbar,  though  in  principle  any 
consistent  set  of  units  may  be  used  for  calibration.    The  factors  CONM,  CONL,  and 
CONT  convert  the  unit  system  of  the  model  being  analyzed  to  the  calibration  unit 
system  in  which  the  Miller’s  extension  parameters  are  specified,  e.g.    a  mass  value  in 
model  units  may  be  multiplied  by  CONM  to  obtain  the  corresponding  value  in 
calibration  units.    These  conversion  factors  allow  consistent  evaluation  of  the  growth 
equation  in  the  calibrated  units.    For  user  convenience,  predefined  conversion  factors 
are  provided  for  converting  various  choices  for  the  model  units  system  to  the 
calibration unit system used by Miller and Guirguis. 
The AFTERBURN option introduces an additional 5th history variable that records the 
added  afterburn  energy  𝑄  for  simple  afterburn  (OPT = 1,2),  but  contains  the  growth 
term 𝜆 when using the Miller’s extension model (OPT = 3).
This is Equation of state Form 3. 
*EOS_SACK_TUESDAY 
  Card 1 
1 
Variable 
EOSID 
Type 
A8 
2 
A1 
F 
3 
A2 
F 
4 
A3 
F 
5 
B1 
F 
6 
B2 
F 
7 
E0 
F 
8 
V0 
F 
  VARIABLE   
EOSID 
DESCRIPTION
Equation  of  state  ID,  a  unique  number  or  label  not  exceeding  8
characters must be specified. 
Ai, Bi 
Constants in the equation of state 
E0 
V0 
Initial internal energy 
Initial relative volume 
Remarks: 
The Sack equation of state defines pressure as 
𝑝 =
𝐴3
𝑉𝐴1
𝑒−𝐴2𝑉 (1 −
𝐵1
) +
𝐵2
𝐸 
and is used for detonation products of high explosives.
This is Equation of state Form 4. 
*EOS 
  Card 1 
1 
Variable 
EOSID 
Type 
A8 
  Card 2 
Variable 
1 
V0 
Type 
F 
  VARIABLE   
EOSID 
2 
C 
F 
2 
3 
S1 
F 
3 
4 
S2 
F 
4 
5 
S3 
F 
5 
6 
GAMAO 
F 
6 
7 
A 
F 
7 
8 
E0 
F 
8 
DESCRIPTION
Equation of state ID, a unique number or label not exceeding 8
characters must be specified. 
C, Si, GAMMA0 
Constants in the equation of state 
First order volume correction coefficient 
Initial internal energy 
Initial relative volume 
A 
E0 
V0 
Remarks: 
The  Gruneisen  equation  of  state  with  cubic  shock-velocity  as  a  function  of  particle-
velocity 𝑣𝑠(𝑣𝑝) defines pressure for compressed materials as 
𝜌0𝐶2𝜇[1 + (1 −
)𝜇 − 𝑎
𝜇2]
𝑝 =
𝛾0
𝜇2
𝜇 + 1
− 𝑆3
𝜇3
(𝜇 + 1)2]
[1 − (𝑆1 − 1)𝜇 − 𝑆2
and for expanded materials as  
2 + (𝛾0 + 𝑎𝜇)𝐸. 
𝑝 = 𝜌0𝐶2𝜇 + (𝛾0 + 𝑎𝜇)𝐸.
where  C  is  the  intercept  of  the  𝑣𝑠(𝑣𝑝)  curve  (in  velocity  units);  S1,  S2,  and  S3  are  the 
unitless coefficients of the slope of the 𝑣𝑠(𝑣𝑝) curve; γ
0 is the unitless Gruneisen gamma; 
a is the unitless, first order volume correction to γ
0; and 
𝜇 =
𝜌0
− 1.
This is Equation of state Form 5. 
*EOS 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EOSID 
Type 
A8 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
A10 
Type 
F 
A11 
F 
A12 
F 
A13 
F 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
A20 
Type 
F 
A21 
F 
A22 
F 
A23 
F 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
A30 
Type 
F 
A31 
F 
A32 
F 
A33 
F 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
A40 
Type 
F 
A41 
F 
A42 
F 
A43
Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
A50 
Type 
F 
A51 
F 
A52 
F 
A53 
F 
  Card 7 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
A60 
Type 
F 
A61 
F 
A62 
F 
A63 
F 
  Card 8 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
A70 
Type 
F 
A71 
F 
A72 
F 
A73 
F 
  Card 9 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
A14 
Type 
F 
A24 
F 
  Card 10 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ALPH 
Type 
F 
BETA 
F 
E0 
F 
V0 
F 
  VARIABLE   
EOSID 
DESCRIPTION
Equation  of  state  ID,  a  unique  number  or  label  not  exceeding  8 
characters must be specified. 
Aij 
Polynomial coefficients
VARIABLE   
DESCRIPTION
α 
β 
Initial internal energy 
Initial relative volume 
ALPHA 
BETA 
E0 
V0 
Remarks: 
The ratio of polynomials equation of state defines the pressure as 
where 
𝑝 =
𝐹1 + 𝐹2𝐸 + 𝐹3𝐸2 + 𝐹4𝐸3
𝐹5 + 𝐹6𝐸 + 𝐹7𝐸2
(1 + 𝛼𝜇) 
𝐹𝑖 = ∑ 𝐴𝑖𝑗𝜇𝑗
𝑗=0
,
𝑛 = {
𝑖 < 3
𝑖 ≥ 3
𝜌0
′ = 𝐹1 + 𝛽𝜇2.  By setting coefficient 𝐴10 = 1.0, 
In expanded elements 𝐹1 is replaced by 𝐹1
the delta-phase pressure modeling for this material will be initiated.  The code will reset 
it to 0.0 after setting flags.
− 1 
𝜇 =
*EOS_LINEAR_POLYNOMIAL_WITH_ENERGY_LEAK 
This is Equation of state Form 6. 
  Define  coefficients  for  a  linear  polynomial  EOS,  and  initialize  the 
Purpose: 
thermodynamic 
state of the material by defining E0 and V0 below.  Energy deposition is prescribed via a 
curve. 
  Card 1 
1 
Variable 
EOSID 
Type 
A8 
  Card 2 
Variable 
1 
E0 
Type 
F 
  VARIABLE   
EOSID 
4 
C2 
F 
4 
5 
C3 
F 
5 
6 
C4 
F 
6 
7 
C5 
F 
7 
8 
C6 
F 
8 
2 
C0 
F 
2 
V0 
F 
3 
C1 
F 
3 
LCID 
I 
DESCRIPTION
Equation  of  state  ID,  a  unique  number  or  label  not  exceeding  8
characters must be specified. 
Ci 
E0 
V0 
Constants in the equation of state 
Initial internal energy 
Initial relative volume 
LCID 
Load curve ID defining the energy deposition rate. 
Remarks: 
This polynomial equation of state, linear in the internal energy per initial volume, 𝐸, is 
given by 
𝑝 = 𝐶0 + 𝐶1𝜇 + 𝐶2𝜇2 + 𝐶3𝜇3 + (𝐶4 + 𝐶5𝜇 + 𝐶6𝜇2)𝐸 
in which 𝐶1, 𝐶2, 𝐶3, 𝐶4, 𝐶5, and 𝐶6 are user defined constants and
where 𝑉 is the relative volume.  In expanded elements, we set the coefficients of 𝜇2 to 
zero, i.e., 
− 1  . 
𝜇 =   
Internal energy, 𝐸, is increased according to an energy deposition rate versus time curve 
whose ID is defined in the input.
𝐶2 = 𝐶6 = 0
*EOS_IGNITION_AND_GROWTH_OF_REACTION_IN_HE 
This is Equation of state Form 7. 
  Card 1 
1 
Variable 
EOSID 
Type 
A8 
  Card 2 
Variable 
1 
R2 
Type 
F 
  Card 3 
1 
2 
A 
F 
2 
R3 
F 
2 
3 
B 
F 
3 
R5 
F 
3 
4 
5 
6 
XP1 
XP2 
FRER 
F 
5 
F 
6 
7 
G 
F 
7 
8 
R1 
F 
8 
FMXIG 
FREQ 
GROW1 
EM 
F 
5 
F 
6 
F 
7 
F 
8 
F 
4 
R6 
F 
4 
Variable 
AR1 
ES1 
CVP 
CVR 
EETAL 
CCRIT 
ENQ 
TMP0 
Type 
F 
  Card 4 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
GROW2 
AR2 
ES2 
EN 
FMXGR 
FMNGR 
Type 
F 
F 
F 
F 
F 
F 
  VARIABLE   
EOSID 
DESCRIPTION
Equation  of  state  ID,  a  unique  number  or  label  not  exceeding  8 
characters must be specified. 
A 
B 
Product JWL constant  
Product JWL constant  
XP1 
Product JWL constant
VARIABLE   
DESCRIPTION
XP2 
FRER 
G 
R1 
R2 
R3 
R5 
R6 
Product JWL constant  
Constant in ignition term of reaction equation 
𝜔𝐶𝑣 of product 
Unreacted JWL constant  
Unreacted JWL constant  
𝜔𝐶𝑣 of unreacted explosive 
Unreacted JWL constant  
Unreacted JWL constant  
FMXIG 
Maximum F for ignition term 
FREQ 
Constant in ignition term of reaction equation 
GROW1 
Constant in growth term of reaction equation 
EM 
AR1 
ES1 
CVP 
CVR 
Constant in growth term of reaction equation 
Constant in growth term of reaction equation 
Constant in growth term of reaction equation 
Heat capacity of reaction products 
Heat capacity of unreacted HE 
EETAL 
Constant in ignition term of reaction equation 
CCRIT 
Constant in ignition term of reaction equation 
ENQ 
TMP0 
Heat of reaction 
Initial temperature (°K) 
GROW2 
Constant in completion term of reaction equation 
AR2 
ES2 
EN 
Constant in completion term of reaction equation 
Constant in completion term of reaction equation 
Constant in completion term of reaction equation
VARIABLE   
DESCRIPTION
FMXGR 
Maximum F for growth term 
FMNGR 
Maximum F for completion term 
Remarks: 
Equation of State Form 7 is used to calculate the shock initiation (or failure to initiate) 
and detonation wave propagation of solid high explosives.  It should be used instead of 
the ideal HE burn options whenever there is a question whether the HE will react, there 
is  a  finite  time  required  for  a  shock  wave  to  build  up  to  detonation,  and/or  there  is  a 
finite  thickness  of  the  chemical  reaction  zone  in  a  detonation  wave.    At  relatively  low 
initial pressures (<2-3 GPa), this equation of state should be used with material type 10 
for  accurate  calculations  of  the  unreacted  HE  behavior.    At  higher  initial  pressures, 
material  type  9  can  be  used.    A  JWL  equation  of  state  defines  the  pressure  in  the 
unreacted explosive as 
𝑃𝑒 = 𝑟1𝑒−𝑟5𝑉𝑒 + 𝑟2𝑒−𝑟6𝑉𝑒 + 𝑟3
𝑇𝑒
𝑉𝑒
,
(𝑟3 = 𝜔𝑒Cvr) 
where 𝑉𝑒 and 𝑇𝑒 are the relative volume and temperature, respectively, of the unreacted 
explosive.  Another JWL equation of state defines the pressure in the reaction products 
as 
𝑃𝑝 = 𝑎𝑒−𝑥𝑝1𝑉𝑝 + 𝑏𝑒−𝑥𝑝2𝑉𝑝 +
𝑔𝑇𝑝
𝑉𝑝
,
(𝑔 = 𝜔𝑝Cvp) 
where 𝑉𝑝 and 𝑇𝑝 are the relative volume and temperature, respectively, of the reaction 
products.  As the chemical reaction converts unreacted explosive to reaction products, 
these  JWL  equations  of  state  are  used  to  calculate  the  mixture  of  unreacted  explosive 
and reaction products defined by the fraction reacted F(F = O implies no reaction, F = 1 
implies  complete  reaction).    The  temperatures  and  pressures  are  assumed  to  be  equal 
(𝑇𝑒 = 𝑇𝑝, 𝑝𝑒 = 𝑝𝑝) and the relative volumes are additive, i.e., 
𝑉 = (1 − 𝐹)𝑉𝑒 + 𝐹𝑉𝑝 
The  chemical  reaction  rate  for  conversion  of  unreacted  explosive  to  reaction  products 
consists of three physically realistic terms:  an ignition term in which a small amount of 
explosive reacts soon after the shock wave compresses it; a slow growth of reaction as 
this  initial  reaction  spreads;  and  a  rapid  completion  of  reaction  at  high  pressure  and 
temperature.  The form of the reaction rate equation is 
Ignition
⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞
−1 − 1 − CCRIT)EETAL
= FREQ × (1 − 𝐹)FRER(𝑉𝑒
Growth
⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞
+ GROW1 × (1 − 𝐹)ES1𝐹AR1𝑝EM
𝜕𝐹
𝜕𝑡
+ GROW2 × (1 − 𝐹)ES2𝑓 AR2𝑝EN
⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟
Completion
The  ignition rate  is  set  equal  to  zero  when 𝐹 ≥ FMXIG,  the  growth  rate  is  set  equal  to 
zero when 𝐹 ≥ FMXGR, and the completion rate is set equal to zero when 𝐹 ≤ FMNGR. 
Details of the computational methods and many examples of one and two dimensional 
shock  initiation  and  detonation  wave  calculation  can  be  found  in  the  references 
(Cochran  and  Chan  [1979],  Lee  and  Tarver  [1980]). 
  Unfortunately,  sufficient 
experimental  data  has  been  obtained  for  only  two  solid  explosives  to  develop  very 
reliable shock initiation models:  PBX-9504 (and the related HMX-based explosives LX-
14,LX-10,LX-04, etc.) and LX-17 (the insensitive TATB-based explosive).  Reactive flow 
models  have  been  developed  for  other  explosives  (TNT,  PETN,  Composition  B, 
propellants, etc.) but are based on very limited experimental data. 
When this EOS is used with *MAT_009, history variables 4, 7, 9, and 10 are temperature, 
burn fraction, 1/𝑉𝑒, and 1/𝑉𝑝, respectively.  When used with *MAT_010, those histories 
variables  are  incremented  by  1,  i.e.,  history variables  5,  8,  10,  and  11  are  temperature, 
burn  fraction,  1/𝑉𝑒,  and  1/𝑉𝑝,  respectively.    See  NEIPH  in  *DATABASE_EXTENT_BI-
NARY if these output variables are desired in the databases for post-processing.
*EOS_TABULATED_COMPACTION 
This is Equation of state Form 8. 
  Card 1 
1 
2 
Variable 
EOSID 
GAMA 
Type 
A8 
F 
3 
E0 
F 
4 
V0 
F 
5 
6 
7 
8 
LCC 
LCT 
LCK 
I 
I 
I 
Parameter  Card  Pairs.    Include  one  pair  of  the  following  two  cards  for  each  of 
VAR = 𝜀𝑣𝑖
,  𝐶𝑖,  𝑇𝑖,  and  𝐾𝑖.    These  cards  consist  of  four  additional  pairs  for  a  total  of  8 
additional cards. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
[VAR]1 
[VAR]2 
[VAR]3 
[VAR]4 
[VAR]5 
Type 
F 
F 
F 
F 
F 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
[VAR]6 
[VAR]7 
[VAR]8 
[VAR]9 
[VAR]10 
Type 
F 
F 
F 
F 
F 
  VARIABLE 
EOSID 
DESCRIPTION
Equation of state ID, a unique number or label not exceeding 8
characters must be specified. 
GAMA 
𝛾, (unitless), see equation in Remarks. 
E0 
V0 
Initial internal energy per unit reference volume (force per unit
area). 
Initial relative volume (unitless).
VARIABLE 
LCC 
DESCRIPTION
Load  curve  defining  tabulated  function  𝐶.    See  equation  in 
Remarks.    The  abscissa  values  of  LCC,  LCT  and  LCK  must  be
negative  of  the  volumetric  strain  in  monotonically  increasing
order,  in  contrast  to  the  convention  in  EOS_9.    The  definition
can extend into the tensile regime. 
LCT 
Load  curve  defining  tabulated  function  𝑇.    See  equation  in 
Remarks. 
LCK 
Load curve defining tabulated bulk modulus. 
𝜀𝑣1, 𝜀𝑣2
,  …, 𝜀𝑣𝑁 
Volumetric strain, ln(𝑉). The first abscissa point,  EV1, must  be 
0.0 or positive if the curve extends into the tensile regime with
subsequent points decreasing monotonically. 
𝐶1, 𝐶2, …, 𝐶𝑁 
𝐶(𝜀𝑉), (units = force per unit area), see equation in Remarks. 
𝑇1, 𝑇2, …, 𝑇𝑁 
𝑇(𝜀𝑉), (unitless), see equation in Remarks. 
𝐾1, 𝐾2, …, 𝐾𝑁 
Bulk unloading modulus (units = force per unit area).
v6
v5
v4
v3 ε
v2
v1
ln(V/V0)
Figure EOS8-1.  Pressure versus volumetric strain curve for Equation of state
Form 8 with compaction.  In the compacted states the bulk unloading modulus
depends  on  the  peak  volumetric  strain.    Volumetric  strain  values  should  be
input  with  correct  sign  (negative  in  compression)  and  in  descending  order.
Pressure is positive in compression. 
  VARIABLE 
DESCRIPTION
Remarks: 
The tabulated compaction model is linear in internal energy.  Pressure is defined by 
𝑝 = 𝐶(𝜀𝑉) + 𝛾 𝑇(𝜀𝑉)𝐸 
in the loading phase.  The volumetric strain, 𝜀𝑉 is given by the natural logarithm of the 
relative  volume  𝑉.    Unloading  occurs  along  the  unloading  bulk  modulus  to  the 
pressure  cutoff.    The  pressure  cutoff,  a  tension  limit,  is  defined  in  the  material  model 
definition.  Reloading always follows the unloading path to the point where unloading 
began,  and  continues  on  the  loading  path,  see  Figure  EOS8-1.    Up  to  10  points  and  as 
few  as  2  may  be  used  when  defining  the  tabulated  functions.    LS-DYNA  will 
extrapolate to find the pressure if necessary.
This is Equation of state Form 9. 
*EOS 
  Card 1 
1 
2 
Variable 
EOSID 
GAMA 
Type 
A8 
F 
3 
E0 
F 
4 
V0 
F 
5 
6 
7 
8 
LCC 
LCT 
I 
I 
Parameter  Card  Pairs.    Include  one  pair  of  the  following  two  cards  for  each  of 
VAR = 𝜀𝑉𝑖
, 𝐶𝑖, 𝑇𝑖.  These cards consist of three additional pairs for a total of 6 additional 
cards.  These cards are not required if LCC and LCT are specified. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
[VAR]1 
[VAR]2 
[VAR]3 
[VAR]4 
[VAR]5 
Type 
F 
F 
F 
F 
F 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
[VAR]6 
[VAR]7 
[VAR]8 
[VAR]9 
[VAR]10 
Type 
F 
F 
F 
F 
F 
  VARIABLE 
EOSID 
DESCRIPTION
Equation  of  state  ID,  a  unique  number  or  label  not  exceeding  8
characters must be specified. 
GAMA 
𝛾, (unitless) see equation in Remarks. 
E0 
V0 
Initial  internal  energy  per  unit  reference  volume  (force  per  unit
area). 
Initial relative volume (unitless).
VARIABLE 
DESCRIPTION
LCC 
LCT 
Load  curve  defining  tabulated  function  𝐶.    See  equation  in 
Remarks.    The  abscissa  values  of  LCC  and  LCT  must  increase
monotonically.  The definition can extend into the tensile regime.
Load  curve  defining  tabulated  function  𝑇.    See  equation  in 
Remarks. 
𝜀𝑉1, 𝜀𝑉2, …, 𝜀𝑉𝑁 
Volumetric  strain,  ln(𝑉),  where  𝑉  is  the  relative  volume.    The 
first  abscissa  point,  EV1,  must  be  0.0  or  positive  if  the  curve 
extends into the tensile regime with subsequent points decreasing
monotonically. 
𝐶1, 𝐶2, …, 𝐶𝑁 
Tabulated points for function 𝐶 (force per unit area). 
𝑇1, 𝑇2, …, 𝑇𝑁 
Tabulated points for function 𝑇 (unitless). 
Remarks: 
The tabulated equation of state model is linear in internal energy.  Pressure is defined 
by 
𝑃 = 𝐶(𝜀𝑉) + 𝛾𝑇(𝜀𝑉)𝐸 
The volumetric strain, 𝜀𝑉 is given by the natural logarithm of the relative volume 𝑉.  Up 
to  10  points  and  as  few  as  2  may  be  used  when  defining  the  tabulated  functions.    LS-
DYNA will extrapolate to find the pressure if necessary.
*EOS_PROPELLANT_DEFLAGRATION 
This Equation of state (10) has been added to model airbag propellants. 
  Card 1 
1 
Variable 
EOSID 
Type 
A8 
  Card 2 
Variable 
Type 
  Card 3 
Variable 
1 
G 
F 
1 
R6 
2 
A 
F 
2 
R1 
F 
2 
3 
B 
F 
3 
R2 
F 
3 
4 
5 
6 
7 
8 
XP1 
XP2 
FRER 
F 
F 
4 
R3 
F 
4 
5 
R5 
F 
5 
F 
6 
7 
8 
6 
7 
8 
FMXIG 
FREQ 
GROW1 
EM 
Type 
F 
  Card 4 
1 
F 
2 
F 
3 
F 
4 
F 
5 
6 
7 
8 
Variable 
AR1 
ES1 
CVP 
CVR 
EETAL 
CCRIT 
ENQ 
TMP0 
Type 
F 
  Card 5 
1 
F 
2 
F 
3 
F 
4 
F 
5 
6 
7 
8 
Variable 
GROW2 
AR2 
ES2 
EN 
FMXGR 
FMNGR 
Type 
F 
F 
F 
F 
F
EOSID 
*EOS_PROPELLANT_DEFLAGRATION 
DESCRIPTION
Equation  of  state  ID,  a  unique  number  or  label  not  exceeding  8
characters must be specified. 
A 
B 
XP1 
XP2 
Product JWL coefficient 
Product JWL coefficient 
Product JWL coefficient 
Product JWL coefficient 
FRER 
Unreacted Co-volume 
G 
R1 
R2 
R3 
R5 
R6 
FMXIG 
FREQ 
Product 𝜔𝐶𝑣 
Unreacted JWL coefficient 
Unreacted JWL coefficient 
Unreacted 𝜔𝐶𝑣 
Unreacted JWL coefficient 
Unreacted JWL coefficient 
Initial Fraction Reacted 𝐹0 
Initial Pressure 𝑃0 
GROW1 
First burn rate coefficient 
EM 
AR1 
ES1 
CVP 
CVR 
Pressure Exponent (1st term) 
Exponent on 𝐹 (1st term) 
Exponent on (1 − 𝐹) (1st term) 
Heat capacity 𝐶𝑣 for products 
Heat capacity 𝐶𝑣 for unreacted material 
EETAL 
Extra, not presently used 
CCRIT 
Product co-volume 
ENQ 
Heat of Reaction
VARIABLE   
DESCRIPTION
TMP0 
Initial Temperature (298°K) 
GROW2 
Second burn rate coefficient 
AR2 
ES2 
EN 
Exponent on 𝐹 (2nd term) 
Exponent on (1 − 𝐹) (2nd term) 
Pressure Exponent  (2nd term) 
FMXGR 
Maximum 𝐹 for 1st term 
FMNGR 
Minimum 𝐹 for 2nd term 
Remarks: 
A deflagration (burn rate) reactive flow model requires an unreacted solid equation of 
state, a reaction product equation of state, a reaction rate law and a mixture rule for the 
two  (or  more)  species.    The  mixture  rule  for  the  standard  ignition  and  growth  model 
[Lee  and  Tarver  1980]  assumes  that  both  pressures  and  temperatures  are  completely 
equilibrated  as  the  reaction  proceeds.    However,  the  mixture  rule  can  be  modified  to 
allow  no  thermal  conduction  or  partial  heating  of  the  solid  by  the  reaction  product 
gases.    For  this  relatively  slow  process  of  airbag  propellant  burn,  the  thermal  and 
pressure  equilibrium  assumptions  are  valid.    The  equations  of  state  currently  used  in 
the burn model are the JWL, Gruneisen, the van der Waals co-volume, and the perfect 
gas law, but other equations of state can be easily implemented.  In this propellant burn, 
the gaseous nitrogen produced by the burning sodium azide obeys the perfect gas law 
as  it  fills  the  airbag  but  may  have  to  be  modeled  as  a  van  der  Waal’s  gas  at  the  high 
pressures and temperatures produced in the propellant chamber.  The chemical reaction 
rate  law  is  pressure,  particle  geometry  and  surface  area  dependent,  as  are  most  high-
pressure  burn  processes.    When  the  temperature  profile  of  the  reacting  system  is  well 
known, temperature dependent Arrhenius chemical kinetics can be used. 
Since  the  airbag  propellant  composition  and  performance  data  are  company  private 
information,  it  is  very  difficult  to  obtain  the  required  information  for  burn  rate 
modeling.  However, Imperial Chemical Industries (ICI) Corporation supplied pressure 
exponent,  particle  geometry,  packing  density,  heat  of  reaction,  and  atmospheric 
pressure  burn  rate  data  which  allowed  us  to  develop  the  numerical  model  presented 
here  for  their  NaN3  +  Fe2O3  driver  airbag  propellant.    The  deflagration  model,  its 
implementation, and the results for the ICI propellant are presented in [Hallquist, et.al., 
1990].
The  unreacted  propellant  and  the  reaction  product  equations  of  state  are  both  of  the 
form: 
𝑝 = 𝐴𝑒−𝑅1𝑉 + 𝐵𝑒−𝑅2𝑉 +
𝜔𝐶𝑣𝑇
𝑉 − 𝑑
where  𝑝  is  pressure  (in  Mbars),  𝑉  is  the  relative  specific  volume  (inverse  of  relative 
density),  𝜔  is  the  Gruneisen  coefficient,  𝐶𝑣  is  heat  capacity  (in  Mbars  -cc/cc°K),  𝑇  is 
temperature  in  °K,  𝑑  is  the  co-volume,  and  𝐴,  𝐵,  𝑅1  and  𝑅2    are  constants.    Setting 
𝐴 = 𝐵 = 0 yields the van der Waal’s co-volume equation of state.  The JWL equation of 
state is generally useful at pressures above several kilobars, while the van der Waal’s is 
useful at pressures below that range and above the range for which the perfect gas law 
holds.  Additionally, setting 𝐴 = 𝐵 = 𝑑 = 0 yields the perfect gas law.  If accurate values 
of  𝜔  and  𝐶𝑣  plus  the  correct  distribution  between  “cold”  compression  and  internal 
energies are used, the calculated temperatures are very reasonable and thus can be used 
to check propellant performance. 
The reaction rate used for the propellant deflagration process is of the form: 
∂𝐹
∂𝑡
= 𝑍(1 − 𝐹)𝑦𝐹𝑥𝑝𝑤
⏟⏟⏟⏟⏟⏟⏟
0<𝐹<𝐹limit1
+ 𝑉(1 − 𝐹)𝑢𝐹𝑟𝑝𝑠
⏟⏟⏟⏟⏟⏟⏟
𝐹limit2<𝐹<1
where 𝐹 is the fraction reacted (𝐹 = 0 implies no reaction, 𝐹 = 1 is complete reaction), 𝑡 
is time, and 𝑝 is pressure (in Mbars), 𝑟, 𝑠, 𝑢, 𝑤, 𝑥, 𝑦, 𝐹limit1  and 𝐹limit2 are constants used 
to describe the pressure dependence and surface area dependence of the reaction rates.  
Two (or more) pressure dependant reaction rates are included in case the propellant is a 
mixture  or  exhibited  a  sharp  change  in  reaction  rate  at  some  pressure  or temperature.  
Burning  surface  area  dependencies  can  be  approximated  using  the  (1 − 𝐹)𝑦𝐹𝑥  terms.  
Other forms of the reaction rate law, such as Arrhenius temperature dependent 𝑒−𝐸 𝑅𝑇⁄
type  rates,  can  be  used,  but  these  require  very  accurate  temperatures  calculations.  
Although  the  theoretical  justification  of  pressure  dependent  burn  rates  at  kilobar  type 
pressures is not complete, a vast amount of experimental burn rate versus pressure data 
does demonstrate this effect and hydrodynamic calculations using pressure dependent 
burn accurately simulate such experiments. 
The  deflagration  reactive  flow  model  is  activated  by  any  pressure  or  particle  velocity 
increase  on  one  or  more  zone  boundaries  in  the  reactive  material.    Such  an  increase 
creates  pressure  in  those  zones  and  the  decomposition  begins.    If  the  pressure  is 
relieved,  the  reaction  rate  decreases  and  can  go  to  zero.    This  feature  is  important  for 
short  duration,  partial  decomposition  reactions.    If  the  pressure  is  maintained,  the 
fraction  reacted  eventually  reaches  one  and  the  material  is  completely  converted  to 
product  molecules.    The  deflagration  front  rates  of  advance  through  the  propellant 
calculated  by  this  model  for  several  propellants  are  quite  close  to  the  experimentally 
observed burn rate versus pressure curves.
To obtain good agreement with experimental deflagration data, the model requires an 
accurate description of the unreacted propellant equation of state, either an analytical fit 
to experimental compression data or an estimated fit based on previous experience with 
similar materials.  This is also true for the reaction products equation of state.  The more 
experimental  burn  rate,  pressure  production  and  energy  delivery  data  available,  the 
better the form and constants in the reaction rate equation can be determined. 
Therefore, the equations used in the burn subroutine for the pressure in the unreacted 
propellant 
𝑃𝑢 = R1 × 𝑒−R5⋅𝑉𝑢 + R2 × 𝑒−R6⋅𝑉𝑢 +
R3 × 𝑇𝑢
𝑉𝑢 − FRER
where 𝑉𝑢 and 𝑇𝑢 are the relative volume and temperature respectively of the unreacted 
propellant.    The  relative  density  is  obviously  the  inverse  of  the  relative  volume.    The 
pressure 𝑃𝑝 in the reaction products is given by: 
𝑃𝑝 = A× 𝑒−XP1×𝑉𝑝 + B × 𝑒−XP2×𝑉𝑝 +
G×𝑇𝑝
𝑉𝑝 − CCRIT
As  the  reaction  proceeds,  the  unreacted  and  product  pressures  and  temperatures  are 
assumed  to  be  equilibrated  (𝑇𝑢 = 𝑇𝑝 = 𝑇,  𝑃 = 𝑃𝑢 = 𝑃𝑝)  and  the  relative  volumes  are 
additive: 
𝑉 = (1 − 𝐹)𝑉𝑢 + 𝐹𝑉𝑝  
where  𝑉  is  the  total  relative  volume.    Other  mixture  assumptions  can  and  have  been 
used in different versions of DYNA2D/3D.  The reaction rate law has the form: 
𝜕𝐹
𝜕𝑡
= GROW1 × (𝑃 + FREQ)EM(𝐹 + FMXIG)AR1(1 − 𝐹 + FMIXG)ES1
+ GROW2 × (𝑃 + FREQ)EN(𝐹 + FMIXG)AR2(1 − 𝐹 + FMIXG)ES2 
If  𝐹  exceeds  FMXGR,  the  GROW1  term  is  set  equal  to  zero,  and,  if  𝐹  is  less  than 
FMNGR, the GROW2 term is zero.  Thus, two separate (or overlapping) burn rates can 
be used to describe the rate at which the propellant decomposes. 
This equation of state subroutine is used together with a material model to describe the 
propellant.  In the airbag propellant case, a null material model (type #10) can be used.  
Material  type  #10  is  usually  used  for  a  solid  propellant  or  explosive  when  the  shear 
modulus  and  yield  strength  are  defined.    The  propellant  material  is  defined  by  the 
material  model  and  the  unreacted  equation  of  state  until  the  reaction  begins.    The 
calculated  mixture  states  are  used  until  the  reaction  is  complete  and  then  the  reaction 
product  equation  of  state  is  used.    The  heat  of  reaction,  ENQ,  is  assumed  to  be  a 
constant and the same at all values of 𝐹 but more complex energy release laws could be 
implemented.
History variables 4 and 7 are temperature and burn fraction, respectively.  See NEIPH 
in  *DATABASE_EXTENT_BINARY  if  these  output  variables  are  desired  in  the 
databases for post-processing.
This is Equation of state Form 11. 
*EOS 
  Card 1 
1 
2 
3 
4 
5 
Variable 
EOSID 
NLD 
NCR 
MU1 
MU2 
6 
IE0 
7 
EC0 
8 
Type 
A8 
F 
F 
F 
F 
F 
F 
DESCRIPTION
Equation  of  state  ID,  a  unique  number  or  label  not  exceeding  8
characters must be specified. 
Virgin loading load curve ID 
Completely crushed load curve ID 
Excess Compression required before any pores can collapse 
Excess  Compression  point  where  the  Virgin  Loading  Curve  and
the Completely Crushed Curve intersect 
Initial Internal Energy 
Initial Excess Compression 
  VARIABLE   
EOSID 
NLD 
NCR 
MU1 
MU2 
IE0 
EC0 
Remarks: 
The pore collapse model described in the TENSOR manual [23] is no longer valid and 
has  been  replaced  by  a  much  simpler  method.    This  is  due  in  part  to  the  lack  of 
experimental  data  required  for  the  more  complex  model.    It  is  desired  to  have  a  close 
approximation  of  the  TENSOR  model  in  the  DYNA  code  to  enable  a  quality  link 
between  them.    The  TENSOR  model  defines  two  curves,  the  virgin  loading  curve  and 
the  completely  crushed  curve  as  shown  in  Figure  EOS11-1  also  defines  the  excess 
compression point required for pore collapse to begin, 𝜇1, and the excess compression 
point required to completely crush the material, 𝜇2.  From this data and the maximum 
excess  compression  the  material  has  attained,  𝑢max,  the  pressure  for  any  excess 
compression, 𝜇, can be determined.
1.0
.8
.6
.4
.2
(
)
Virgin
loading
curve
Completely
crushed
curve
Partially
crushed
curve
.04
.08
.12
.16
.20
Excess Compression
Figure EOS11-1.  Pressure versus compaction curve 
Unloading occurs along the virgin loading curve until the excess compression surpasses 
𝜇1.  After that, the unloading follows a path between the completely crushed curve and 
the virgin loading curve.  Reloading will follow this curve back up to the virgin loading 
curve.    Once  the  excess  compression  exceeds  𝜇2,  then  all  unloading  will  follow  the 
completely crushed curve. 
For  unloading  between  𝜇1  and    a  partially𝜇2  crushed  curve  is  determined  by  the 
relation: 
where 
𝑝pc(𝜇) = 𝑝cc [
𝜇𝑎
⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞
(1 + 𝜇𝐵)(1 + 𝜇)
− 1]
1 + 𝜇max
. 
𝜇𝐵 = 𝑃cc
−1(𝑃max) 
and the subscripts “pc” and “cc” refer to the partially crushed and completely crushed 
states, respectively.  This is more readily understood in terms of the relative volume, 𝑉. 
𝑉 =
1 + 𝜇
𝑃pc(𝑉) = 𝑃cc (
𝑉𝐵
𝑉min
𝑉)
This representation suggests that for a fixed 
𝑉min =
𝜇max + 1
the partially crushed curve will separate linearly from the completely crushed curve as 
𝑉 increases to account for pore recovery in the material. 
The bulk modulus 𝐾 is determined to be the slope of the current curve times one plus 
the excess compression 
𝐾 =
∂𝑃
∂𝜇
(1 + 𝜇) 
The slope ∂𝑃
∂𝜇 for the partially crushed curve is obtained by differentiation as: 
𝜕𝑝pc
𝜕𝜇
=
𝜕𝑝cc
𝜕𝑥
∣
𝑥=
(1+𝜇𝑏)(1+𝜇)
1+𝜇max
−1
(
1 + 𝜇𝑏
1 + 𝜇max
) 
Simplifying, 
where 
𝐾 =
∂𝑃cc
∂𝜇𝑎
∣
μa
(1 + 𝜇𝑎) 
𝜇𝑎 =
(1 + 𝜇𝐵)(1 + 𝜇)
(1 + 𝜇max)
− 1. 
The bulk sound speed is determined from the slope of the completely crushed curve at 
the current pressure to avoid instabilities in the time step. 
The virgin loading and completely crushed curves are modeled with monotonic cubic-
splines.    An  optimized  vector  interpolation scheme  is  then  used  to  evaluate  the  cubic-
splines.  The bulk modulus and sound speed are derived from a linear interpolation on 
the derivatives of the cubic-splines.
*EOS_IDEAL_GAS 
Purpose:    This  is  equation  of  state  form  12  for  modeling  ideal  gas.    It  is  an  alternate 
approach  to  using  *EOS_LINEAR_POLYNOMIAL  with  C4 = C5 = (𝛾 − 1)  to  model 
ideal gas.  This has a slightly improved energy accounting algorithm. 
  Card 1 
1 
2 
3 
Variable 
EOSID 
CV0 
CP0 
4 
CL 
F 
4 
5 
CQ 
F 
5 
6 
T0 
F 
6 
7 
V0 
F 
7 
8 
VCO 
F 
8 
F 
2 
F 
3 
Type 
A8 
  Card 2 
1 
Variable 
ADIAB 
Type 
F 
  VARIABLE   
EOSID 
CV0 
CP0 
CL 
CQ 
T0 
V0 
DESCRIPTION
Equation  of  state  ID,  a  unique  number  or  label  not  exceeding  8
characters must be specified. 
Nominal constant-volume specific heat coefficient (at STP) 
Nominal constant-pressure specific heat coefficient (at STP) 
Linear coefficient for the variations of 𝐶𝑣 and 𝐶𝑝versus 𝑇. 
Quadratic coefficient for the variations of 𝐶𝑣 and 𝐶𝑝 versus 𝑇. 
Initial temperature 
Initial relative volume  
VCO 
Van der Waals covolume 
ADIAB 
Adiabatic flag: 
EQ.0.0:  off 
EQ.1.0:  on; ideal gas follows adiabatic law
1.  The pressure in the ideal gas law is defined as 
*EOS 
𝑝 = 𝜌(𝐶𝑝 − 𝐶𝑣)𝑇 
𝐶𝑝 = 𝐶𝑝0 + 𝐶𝐿𝑇 + 𝐶𝑄𝑇2 
𝐶𝑣 = 𝐶𝑣0 + 𝐶𝐿𝑇 + 𝐶𝑄𝑇2 
where  𝐶𝑝  and  𝐶𝑣  are  the  specific  heat  capacities  at  constant  pressure  and  at 
constant volume, respectively. 𝜌 is the density.  The relative volume is defined 
as 
𝜐𝑟 =
𝑉0
=
)
(𝑉 𝑀⁄
)
(𝑉0 𝑀⁄
=
𝜐0
=
𝜌0
where  𝜌0  is  a  nominal  or  reference  density  defined  in  the  *MAT_NULL  card.  
The initial pressure can then be manually computed as 
𝑃|𝑡=0    =    𝜌∣𝑡=0(𝐶𝑃 − 𝐶𝑉)𝑇|𝑡=0 
𝜌∣𝑡=0 = {
𝑃|𝑡=0    = {
𝜌0
𝜐𝑟|𝑡=0
𝜌0
𝜐𝑟|𝑡=0
} 
} (𝐶𝑃 − 𝐶𝑉)𝑇|𝑡=0 
The  initial  relative  volume,  𝜐𝑟|𝑡=0  (V0),  initial  temperature,  𝑇|𝑡=0(T0),  and  heat 
capacity information are defined in the *EOS_IDEAL_GAS input.  Note that the 
“reference”  density  is  typically  a  density  at  a  non-stressed  or  nominal  stress 
state.  The initial pressure should always be checked manually against simula-
tion result. 
2.  With  adiabatic  flag  on,  the  adiabatic  state  is  conserved,  but  extact  internal 
energy conservation is scarified. 
3.  The ideal gas model is good for low density gas only.  Deviation from the ideal 
gas behavior may be indicated by the compressibility factor defined as 
𝑍 =
𝑃𝜐
𝑅𝑇
When 𝑍 deviates from 1, the gas behavior deviates from ideal. 
4.  V0 and T0 defined in this card must be the same as the time-zero ordinates for 
the  2  load  curves  defined  in  the  *BOUNDARY_AMBIENT_EOS  card,  if  it  is 
used.  This is so that they both would consistently define the same initial state 
for a material.
*EOS_JWLB 
This  is  Equation  of  state  Form  14.    The  JWLB  (Jones-Wilkens-Lee-Baker)  equation  of 
state,  developed  by  Baker  [1991]  and  further  described  by  Baker  and  Orosz  [1991], 
describes the high pressure regime produced by overdriven detonations while retaining 
the low pressure expansion behavior required for standard acceleration modeling.  The 
derived form of the equation of state is based on the JWL form due to its computational 
robustness  and  asymptotic  approach  to  an  ideal  gas  at  high  expansions.    Additional 
exponential terms and a variable Gruneisen parameter have been added to adequately 
describe the high-pressure region above the Chapman-Jouguet state. 
  Card 1 
1 
Variable 
EOSID 
Type 
A8 
  Card 2 
Variable 
1 
R1 
Type 
F 
  Card 3 
1 
2 
A1 
F 
2 
R2 
F 
2 
3 
A2 
F 
3 
R3 
F 
3 
4 
A3 
F 
4 
R4 
F 
4 
5 
A4 
F 
5 
R5 
F 
5 
Variable 
AL1 
AL2 
AL3 
AL4 
AL5 
Type 
F 
  Card 4 
1 
F 
2 
F 
3 
F 
4 
F 
5 
Variable 
BL1 
BL2 
BL3 
BL4 
BL5 
Type 
F 
F 
F 
F 
F 
6 
A5 
F 
6 
7 
8 
7 
8 
6 
7 
8 
6 
7
Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RL1 
RL2 
RL3 
RL4 
RL5 
Type 
F 
  Card 6 
Variable 
Type 
1 
C 
I 
F 
2 
OMEGA 
F 
F 
3 
E 
F 
F 
4 
V0 
F 
F 
5 
6 
7 
8 
  VARIABLE   
EOSID 
DESCRIPTION 
Equation  of  state  ID,  a  unique  number  or  label  not
exceeding 8 characters must be specified. 
Ai, Ri, Ali, BLi, C, OMEGA 
Equation of state coefficients  𝐴𝑖, 𝑅𝑖,  𝐴𝜆𝑖, 𝐵𝜆𝑖, 𝑅𝜆𝑖,  𝐶, 
𝜔 respectively.  See below. 
C 
Equation of state coefficient, see below. 
OMEGA 
Equation of state coefficient, see below. 
E 
V0 
Energy density per unit initial volume 
Initial relative volume. 
Remarks: 
The JWLB equation-of-state defines the pressure as 
𝑝 = ∑ 𝐴𝑖
𝑖=1
(1 −
𝑅𝑖𝑉
) 𝑒−𝑅𝑖𝑉 +
𝜆𝐸
+ 𝐶 (1 −
) 𝑉−(𝜔+1) 
𝜆 = ∑(𝐴𝜆𝑖𝑉 + 𝐵𝜆𝑖)𝑒−𝑅𝜆𝑖𝑉 + 𝜔
𝑖=1
where V is the relative volume, E is the energy per unit initial volume, and 𝐴𝑖, 𝑅𝑖, 𝐴𝜆𝑖, 
𝐵𝜆𝑖, 𝑅𝜆𝑖, 𝐶, and 𝜔 are input constants defined above. 
JWLB  input  constants  for  some  common  explosives  as  found  in  Baker  and Stiel  [1997] 
are given in the following table.
E0 (Mbar) 
DCJ (cm/μs) 
PCJ (Mbar) 
A1 (Mbar) 
A2 (Mbar) 
A3 (Mbar) 
A4 (Mbar) 
R1 
R2 
R3 
R4 
C (Mbar) 
ω 
Aλ1 
Bλ1 
Rλ1 
Aλ2 
Bλ2 
Rλ2 
TATB 
1.800 
.07040 
.76794 
.23740 
550.06 
22.051 
.42788 
.28094 
16.688 
6.8050 
2.0737 
2.9754 
.00776 
.27952 
1423.9 
14387. 
19.780 
5.0364 
-2.6332 
1.7062 
LX-14 
1.821 
.10205 
.86619 
.31717 
549.60 
64.066 
2.0972 
.88940 
34.636 
8.2176 
20.401 
2.0616 
.01251 
.38375 
18307. 
1390.1 
19.309 
4.4882 
-2.6181 
1.5076 
PETN 
1.765 
.10910 
.83041 
.29076 
521.96 
71.104 
4.4774 
.97725 
44.169 
8.7877 
25.072 
2.2251 
.01570 
.32357 
12.257 
52.404 
43.932 
8.6351 
-4.9176 
2.1303 
*EOS_JWLB 
Octol 70/30 
1.803 
.09590 
.82994 
.29369 
526.83 
60.579 
.91248 
.00159 
52.106 
8.3998 
2.1339 
.18592 
.00968 
.39023 
.011929 
18466. 
20.029 
5.4192 
-3.2394 
1.5868 
TNT 
1.631 
.06656 
.67174 
.18503 
490.07 
56.868 
.82426 
.00093 
40.713 
9.6754 
2.4350 
.15564 
.00710 
.30270 
.00000 
1098.0 
15.614 
11.468 
-6.5011 
2.1593
*EOS 
This  is  Equation  of  state  Form  15.    This  EOS  works  with  solid  elements  and  the  thick 
shell using selective reduced 2 × 2 integration (ELFORM = 2 on SECTION_TSHELL) to 
model the response of gaskets.  For the thick shell only, it is completely decoupled from 
the shell material, i.e., in the local coordinate system of the shell, this model defines the 
normal stress, 𝜎𝑧𝑧, and does not change any of the other stress components. The model 
is a reduction of the *MAT_GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EOSID 
LCID1 
LCID2 
LCID3 
LCID4 
Type 
A8 
  Card 2 
1 
Variable 
UNLOAD 
Type 
F 
I 
2 
K 
F 
I 
3 
I 
4 
I 
5 
6 
7 
8 
DMPF 
TFS 
CFS 
LOFFSET 
IVS 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
EOSID 
LCID1 
LCID2 
LCID3 
LCID4 
Equation  of  state  ID,  a  unique  number  or  label  not  exceeding  8 
characters must be specified. 
Load curve for loading. 
Load curve for unloading. 
Load curve for damping as a function of volumetric strain rate. 
Load  curve  for  scaling  the  damping  as  a  function  of  the
volumetric strain.
*EOS 
Unload = 0
Loading-unloading
curve
Unload = 2
Unloading
curve
*EOS_GASKET 
Unloading
curve
ρ∕ρ
μ = 
0 − 1
Unload = 1
Unload = 3
ρ∕ρ
μ = 
0 − 1
ρ∕ρ
μ = 
0 − 1
umin
× OFFSET
umin
Quadratic
unloading
ρ∕ρ
μ = 
0 − 1
Figure EOS15-1.  Load and unloading behavior. 
  VARIABLE   
DESCRIPTION
UNLOAD 
Unloading option :  
EQ.0.0: Loading and unloading follow loading curve 
EQ.1.0: Loading  follows  loading  curve,  unloading  follows
unloading curve.  The unloading curve ID if undefined
is taken as the loading curve. 
EQ.2.0: Loading  follows  loading  curve,  unloading  follows
unloading  stiffness,  K,  to  the  unloading  curve.    The
loading and unloading curves may only intersect at the 
origin of the axes. 
EQ.3.0: Quadratic unloading from peak displacement value to
DESCRIPTION
a permanent offset. 
K 
Unloading stiffness, for UNLOAD = 2 only. 
*EOS 
DMPF 
TFS 
CFS 
OFFSET 
Damping factor for stability.  Values in the neighborhood of unity
are  recommended.    The  damping  factor  is  properly  scaled  to
eliminate time step size dependency.  
Tensile failure strain. 
Compressive failure strain. 
Offset factor between 0 and 1.0 to determine permanent set upon 
  The  permanent  sets  in 
unloading  if  the  UNLOAD = 3.0. 
compression  and  tension  are  equal  to  the  product  of  this  offset
value  and  the  maximum  compressive  and  tensile  displacements,
respectively. 
IVS 
Initial volume strain.
*EOS_MIE_GRUNEISEN 
This  is  Equation  of  state  Form  16,  a  Mie-Gruneisen  form  with  a  𝑝 − 𝛼  compaction 
model. 
  Card 1 
1 
2 
Variable 
EOSID 
GAMMA 
Type 
A8 
F 
3 
A1 
F 
4 
A2 
F 
5 
A3 
F 
6 
7 
PEL 
PCO 
F 
F 
8 
N 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
4 
5 
6 
7 
8 
  Card 2 
1 
Variable 
ALPHA0 
Type 
F 
2 
E0 
F 
3 
V0 
F 
Default 
none 
none 
none 
  VARIABLE   
EOSID 
DESCRIPTION
Equation  of  state  identification.    A  unique  number  or  label  not
exceeding 8 characters must be specified. 
GAMMA 
Gruneisen gamma. 
Ai 
PEL 
PCO 
N 
Hugoniot polynomial coefficient 
Crush pressure 
Compaction pressure 
Porosity exponent 
ALPHA0 
Initial porosity 
E0 
V0 
Initial internal energy 
Initial relative volume
*EOS 
The equation of state is a Mie-Gruneisen form with a polynomial Hugoniot curve and a 
𝑝 − 𝛼 compaction model.  First, we define a history variable representing the porosity 𝛼 
that is initialised to 𝛼0 > 1. The evolution of this variable is given as 
𝛼(𝑡) = max
⎜⎛1 + (𝛼0 − 1) [
⎝
where 𝑝(𝑡) indicates the pressure at time t.  For later use, we define the cap pressure as 
⎡𝛼0, min𝑠≤𝑡
⎢
⎣
1, min
⎟⎞
⎠
𝑝comp − 𝑝(𝑠)
]
𝑝comp − 𝑝𝑒𝑙
}⎫
⎤
⎥
⎭}⎬
⎦
{⎧
⎩{⎨
𝑝𝑐 = 𝑝comp − (𝑝comp − 𝑝𝑒𝑙) [
1/𝑁
𝛼 − 1
𝛼0 − 1
]
The remainder of the EOS model is given by the equations 
together with  
𝑝(𝜌, 𝑒) = Γ𝛼𝜌𝑒 + 𝑝𝐻(𝜂) [1 −
Γ𝜂] 
𝑝𝐻(𝜂) = 𝐴1𝜂 + 𝐴2𝜂2 + 𝐴3𝜂3 
𝜂(𝜌) =
𝛼𝜌
𝛼0𝜌0
− 1.
*EOS_GRUNEISEN 
This  is  Equation  of  state  Form  19.    This  EOS  works  with  SPH  elements  to  model  the 
response of fluids. 
  Card 1 
1 
2 
Variable 
EOSID 
GAMMA 
Type 
A8 
F 
3 
K0 
F 
4 
V0 
F 
5 
6 
7 
8 
  VARIABLE   
EOSID 
DESCRIPTION
Equation of state ID, a unique number or label not exceeding 8 
characters must be specified. 
GAMMA, K0 
Constants in the equation of state. 
V0 
Initial relative volume. 
Remarks: 
The Murnaghan equation of state defines pressure as 
𝑝 = 𝑘0 [(
𝜌0
)
− 1].
*EOS 
These are equations of state 21-30.  The user can supply his own subroutines.  See also 
Appendix B.  The keyword input has to be used for the user interface with data. 
  Card 1 
1 
2 
3 
4 
5 
Variable 
EOSID 
EOST 
LMC 
NHV 
IVECT 
Type 
A8 
I 
I 
I 
I 
Define LMC material parameters using 8 parameters per card.  
  Card 2 
Variable 
1 
P1 
Type 
F 
2 
P2 
F 
3 
P3 
F 
4 
P4 
F 
5 
P5 
F 
6 
EO 
F 
6 
P6 
F 
7 
VO 
F 
7 
P7 
F 
8 
BULK 
F 
8 
P8 
F 
  VARIABLE   
EOSID 
EOST 
LMC 
DESCRIPTION
Equation  of  state  ID,  a  unique  number  or  label  not  exceeding  8
characters must be specified. 
User equation of state type (21-30 inclusive).  A number between 
21 and 30 has to be chosen. 
Length of material constant array which is equal to the number of
material constants to be input.  (LMC ≤ 48) 
NHV 
Number of history variables to be stored, see Appendix B. 
IVECT 
EO 
V0 
BULK 
Vectorization flag (on = 1).  A vectorized user subroutine must be 
supplied. 
Initial internal energy. 
Initial relative volume. 
Bulk modulus.  This value is used in the calculation of the contact
surface stiffness. 
Pi 
Material  parameters 𝑖 = 1, … ,LMC.
*MAT 
LS-DYNA  has  historically  referenced  each  material  model  by  a  number.    As  shown 
below,  a  three  digit  numerical  designation  can  still  be  used,  e.g.,  *MAT_001,  and  is 
equivalent to a corresponding descriptive designation, e.g., *MAT_ELASTIC.  The two 
equivalent commands for each material model, one numerical and the other descriptive, 
are listed below.  The numbers in square brackets  identify the element 
formulations  for  which  the  material  model  is  implemented.    The  number  in  the  curly 
brackets,  {n},  indicates  the  default  number  of  history variables  per  element  integration 
point that are stored in addition to the 7 history variables which are stored by default.     
Just  as  an  example,  for  the  type  16  fully  integrated  shell  elements  with  2  integration 
points  through  the  thickness,  the  total  number  of  history  variables  is  8 × (𝑛 + 7).    For 
the Belytschko-Tsay type 2 element the number is 2 × (𝑛 + 7).   
The meaning associated with particular extra history variables for a subset of material 
models and equations of state are  tabulated at http://www.dynasupport.com/howtos-
/material/history-variables. 
An  additional  option TITLE  may  be  appended  to  a  *MAT  keyword  in  which  case  an 
additional  line  is  read  in  80a  format  which  can  be  used  to  describe  the  material.    At 
present,  LS-DYNA  does  not  make  use  of  the  title.    Inclusion  of  titles  simply  gives 
greater clarity to input decks. 
Key to numbers in square brackets 
0 
13,14,15) 
1H 
1B 
1I 
1T 
1D 
1SW 
2 
3a 
3c 
4 
5 
6 
7 
8A 
- 
- 
- 
- 
- 
- 
- 
- 
- 
- 
- 
- 
- 
- 
- 
Solids  (and  2D  continuum  elements,  i.e.,  shell  formulations 
Hughes-Liu beam 
Belytschko resultant beam 
Belytschko integrated solid and tubular beams 
Truss 
Discrete beam 
Spotweld beam 
Shells 
Thick shell formulations 1,2,6 
Thick shell formulations 3,5,7 
Special airbag element 
SPH element 
Acoustic solid 
Cohesive solid 
Multi-material ALE solid (validated)
8B 
9 
- 
- 
Multi-material ALE solid (implemented but not validated1) 
Membrane element 
*MAT_ADD_COHESIVE2 [7] {see associated material model} 
*MAT_ADD_EROSION2 
*MAT_ADD_FATIGUE 
*MAT_ADD_GENERALIZED_DAMAGE2 [2] 
*MAT_ADD_PERMEABILTY 
*MAT_ADD_PORE_AIR 
*MAT_ADD_THERMAL_EXPANSION2 
*MAT_NONLOCAL2 
*MAT_ELASTIC [0,1H,1B,1I,1T,2,3a,3c,5,8A] {0} 
*MAT_{OPTION}TROPIC_ELASTIC [0,2,3a,3c] {15} 
*MAT_PLASTIC_KINEMATIC [0,1H,1I,1T,2,3a,3c,5,8A] {5} 
*MAT_ELASTIC_PLASTIC_THERMAL [0,1H,1T,2,3a,3c,5,8B] {3} 
*MAT_SOIL_AND_FOAM [0,5,3c,8A] {0} 
*MAT_VISCOELASTIC [0,1H,2,3a,3c,5,8B] {19} 
*MAT_BLATZ-KO_RUBBER [0,2,3ac,8B] {9} 
*MAT_HIGH_EXPLOSIVE_BURN [0,5,3c,8A] {4} 
*MAT_NULL [0,1,2,3c,5,8A] {3} 
*MAT_ELASTIC_PLASTIC_HYDRO_{OPTION} [0,3c,5,8B] {4} 
*MAT_STEINBERG [0,3c,5,8B] {5} 
*MAT_001: 
*MAT_001_FLUID:  *MAT_ELASTIC_FLUID [0,8A] {0} 
*MAT_002: 
*MAT_003: 
*MAT_004: 
*MAT_005: 
*MAT_006: 
*MAT_007: 
*MAT_008: 
*MAT_009: 
*MAT_010: 
*MAT_011: 
*MAT_011_LUND:  *MAT_STEINBERG_LUND [0,3c,5,8B] {5} 
*MAT_012: 
*MAT_013: 
*MAT_014: 
*MAT_015: 
*MAT_016: 
*MAT_017: 
*MAT_018: 
*MAT_019: 
*MAT_020: 
*MAT_021: 
*MAT_022: 
*MAT_023: 
*MAT_024: 
*MAT_025: 
*MAT_026: 
*MAT_027: 
*MAT_028: 
*MAT_029: 
*MAT_030: 
*MAT_ISOTROPIC_ELASTIC_PLASTIC [0,2,3a,3c,5,8B] {0} 
*MAT_ISOTROPIC_ELASTIC_FAILURE [0,3c,5,8B] {1} 
*MAT_SOIL_AND_FOAM_FAILURE [0,3c,5,8B] {1} 
*MAT_JOHNSON_COOK [0,2,3a,3c,5,8A] {6} 
*MAT_PSEUDO_TENSOR [0,3c,5,8B] {6} 
*MAT_ORIENTED_CRACK [0,3c] {14} 
*MAT_POWER_LAW_PLASTICITY [0,1H,2,3a,3c,5,8B] {0} 
*MAT_STRAIN_RATE_DEPENDENT_PLASTICITY [0,2,3a,3c,5,8B] {6} 
*MAT_RIGID [0,1H,1B,1T,2,3a] {0} 
*MAT_ORTHOTROPIC_THERMAL [0,2,3ac] {29} 
*MAT_COMPOSITE_DAMAGE [0,2,3a,3c,5] {12} 
*MAT_TEMPERATURE_DEPENDENT_ORTHOTROPIC [0,2,3ac] {19} 
*MAT_PIECEWISE_LINEAR_PLASTICITY [0,1H,2,3a,3c,5,8A] {5} 
*MAT_GEOLOGIC_CAP_MODEL [0,3c,5] {12} 
*MAT_HONEYCOMB [0,3c] {20} 
*MAT_MOONEY-RIVLIN_RUBBER [0,1T,2,3c,8B] {9} 
*MAT_RESULTANT_PLASTICITY [1B,2] {5} 
*MAT_FORCE_LIMITED [1B] {30} 
*MAT_SHAPE_MEMORY [0,1H,2,3ac,5] {23} 
1  Error  associated  with  advection  inherently  leads  to  state  variables  that  may  be  inconsistent  with 
nonlinear constitutive routines and thus may lead to nonphysical results, nonconservation of energy, and 
even  numerical  instability  in  some  cases.    Caution  is  advised,  particularly  when  using  the  2nd  tier  of 
material  models  implemented  for  ALE  multi-material  solids  (designated  by  [8B])  which  are  largely 
untested as ALE materials. 
2 These commands do not, by themselves, define a material model but rather can be used in certain cases 
to supplement material models
*MAT_FRAZER_NASH_RUBBER_MODEL [0,3c,8B] {9} 
*MAT_031: 
*MAT_LAMINATED_GLASS [2,3a] {0} 
*MAT_032: 
*MAT_BARLAT_ANISOTROPIC_PLASTICITY [0,2,3a,3c] {9} 
*MAT_033: 
*MAT_BARLAT_YLD96 [2,3a] {9} 
*MAT_033_96: 
*MAT_FABRIC [4] {17} 
*MAT_034: 
*MAT_PLASTIC_GREEN-NAGHDI_RATE [0,3c,5,8B] {22} 
*MAT_035: 
*MAT_3-PARAMETER_BARLAT [2,3a] {7} 
*MAT_036: 
*MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLASTIC [2,3a] {9} 
*MAT_037: 
*MAT_BLATZ-KO_FOAM [0,2,3c,8B] {9} 
*MAT_038: 
*MAT_FLD_TRANSVERSELY_ANISOTROPIC [2,3a] {6} 
*MAT_039: 
*MAT_NONLINEAR_ORTHOTROPIC [0,2,3c] {17} 
*MAT_040: 
*MAT_USER_DEFINED_MATERIAL_MODELS [0,1H,1T,1D,2,3a,3c,5,8B] {0} 
*MAT_041-050: 
*MAT_BAMMAN [0,2,3a,3c,5,8B] {8} 
*MAT_051: 
*MAT_BAMMAN_DAMAGE [0,2,3a,3c,5,8B] {10} 
*MAT_052: 
*MAT_CLOSED_CELL_FOAM [0,3c,8B] {0} 
*MAT_053: 
*MAT_ENHANCED_COMPOSITE_DAMAGE [0,2,3c] {20} 
*MAT_054-055: 
*MAT_LOW_DENSITY_FOAM [0,3c,5,8B] {26} 
*MAT_057: 
*MAT_LAMINATED_COMPOSITE_FABRIC [2,3a] {15} 
*MAT_058: 
*MAT_COMPOSITE_FAILURE_{OPTION}_MODEL [0,2,3c,5] {22} 
*MAT_059: 
*MAT_ELASTIC_WITH_VISCOSITY [0,2,3a,3c,5,8B] {8} 
*MAT_060: 
*MAT_ELASTIC_WITH_VISCOSITY_CURVE [0,2,3a,3c,5,8B] {8} 
*MAT_060C: 
*MAT_KELVIN-MAXWELL_VISCOELASTIC [0,3c,5,8B] {14} 
*MAT_061: 
*MAT_VISCOUS_FOAM [0,3c,8B] {7} 
*MAT_062: 
*MAT_CRUSHABLE_FOAM [0,3c,5,8B] {8} 
*MAT_063: 
*MAT_RATE_SENSITIVE_POWERLAW_PLASTICITY [0,2,3a,3c,5,8B] {30} 
*MAT_064: 
*MAT_MODIFIED_ZERILLI_ARMSTRONG [0,2,3a,3c,5,8B] {6} 
*MAT_065: 
*MAT_LINEAR_ELASTIC_DISCRETE_BEAM [1D] {8} 
*MAT_066: 
*MAT_NONLINEAR_ELASTIC_DISCRETE_BEAM [1D] {14} 
*MAT_067: 
*MAT_NONLINEAR_PLASTIC_DISCRETE_BEAM [1D] {25} 
*MAT_068: 
*MAT_SID_DAMPER_DISCRETE_BEAM [1D] {13} 
*MAT_069: 
*MAT_HYDRAULIC_GAS_DAMPER_DISCRETE_BEAM [1D] {8} 
*MAT_070: 
*MAT_CABLE_DISCRETE_BEAM [1D] {8} 
*MAT_071: 
*MAT_CONCRETE_DAMAGE [0,3c,5,8B] {6} 
*MAT_072: 
*MAT_CONCRETE_DAMAGE_REL3 [0,3c,5] {6} 
*MAT_072R3: 
*MAT_LOW_DENSITY_VISCOUS_FOAM [0,3c,8B] {56} 
*MAT_073: 
*MAT_ELASTIC_SPRING_DISCRETE_BEAM [1D] {8} 
*MAT_074: 
*MAT_BILKHU/DUBOIS_FOAM [0,3c,5,8B] {8} 
*MAT_075: 
*MAT_GENERAL_VISCOELASTIC [0,2,3a,3c,5,8B] {53} 
*MAT_076: 
*MAT_HYPERELASTIC_RUBBER [0,2,3c,5,8B] {54} 
*MAT_077_H: 
*MAT_OGDEN_RUBBER [0,2,3c,8B] {54} 
*MAT_077_O: 
*MAT_SOIL_CONCRETE [0,3c,5,8B] {3} 
*MAT_078: 
*MAT_HYSTERETIC_SOIL [0,3c,5,8B] {96} 
*MAT_079: 
*MAT_RAMBERG-OSGOOD [0,3c,8B] {18} 
*MAT_080: 
*MAT_081: 
*MAT_PLASTICITY_WITH_DAMAGE [0,2,3a,3c] {5} 
*MAT_082(_RCDC):  *MAT_PLASTICITY_WITH_DAMAGE_ORTHO(_RCDC) [0,2,3a,3c] {22} 
*MAT_083: 
*MAT_084: 
*MAT_086: 
*MAT_087: 
*MAT_088: 
*MAT_089: 
*MAT_090: 
*MAT_091: 
*MAT_092: 
*MAT_FU_CHANG_FOAM [0,3c,5,8B] {54} 
*MAT_WINFRITH_CONCRETE [0] {54} 
*MAT_ORTHOTROPIC_VISCOELASTIC [2,3a] {17} 
*MAT_CELLULAR_RUBBER [0,3c,5,8B] {19} 
*MAT_MTS [0,2,3a,3c,5,8B] {5} 
*MAT_PLASTICITY_POLYMER [0,2,3a,3c] {46} 
*MAT_ACOUSTIC [6] {25} 
*MAT_SOFT_TISSUE [0,2] {16} 
*MAT_SOFT_TISSUE_VISCO [0,2] {58}
*MAT_094: 
*MAT_095: 
*MAT_096: 
*MAT_097: 
*MAT_098: 
*MAT_099: 
{22} 
*EOS_USER_DEFINED 
*MAT_ELASTIC_6DOF_SPRING_DISCRETE_BEAM [1D] {25} 
*MAT_INELASTIC_SPRING_DISCRETE_BEAM [1D] {9} 
*MAT_INELASTIC_6DOF_SPRING_DISCRETE_BEAM [1D] {25} 
*MAT_BRITTLE_DAMAGE [0,8B] {51} 
*MAT_GENERAL_JOINT_DISCRETE_BEAM [1D] {23} 
*MAT_SIMPLIFIED_JOHNSON_COOK [0,1H,1B,1T,2,3a,3c] {6} 
*MAT_SIMPLIFIED_JOHNSON_COOK_ORTHOTROPIC_DAMAGE 
[0,2,3a,3c] 
*MAT_100: 
*MAT_100_DA: 
*MAT_101: 
*MAT_102(_T): 
*MAT_103: 
*MAT_103_P: 
*MAT_104: 
*MAT_105: 
*MAT_106: 
*MAT_107: 
*MAT_108: 
*MAT_110: 
*MAT_111: 
*MAT_112: 
*MAT_113: 
*MAT_114: 
*MAT_115: 
*MAT_115_O: 
*MAT_116: 
*MAT_117: 
*MAT_118: 
*MAT_119: 
*MAT_120: 
*MAT_120_JC: 
*MAT_120_RCDC: 
*MAT_121: 
*MAT_122: 
*MAT_122_3D: 
*MAT_123: 
*MAT_124: 
*MAT_125: 
*MAT_126: 
*MAT_127: 
*MAT_128: 
*MAT_129: 
*MAT_130: 
*MAT_131: 
*MAT_132: 
*MAT_133: 
*MAT_134: 
*MAT_135: 
*MAT_135_PLC: 
*MAT_136: 
*MAT_138: 
*MAT_139: 
*MAT_140: 
*MAT_SPOTWELD_{OPTION} [0,1SW] {6} 
*MAT_SPOTWELD_DAIMLERCHRYSLER [0] {6} 
*MAT_GEPLASTIC_SRATE_2000a [2,3a] {15} 
*MAT_INV_HYPERBOLIC_SIN(_THERMAL) [0,3c,8B] {15} 
*MAT_ANISOTROPIC_VISCOPLASTIC [0,2,3a,3c,5] {20} 
*MAT_ANISOTROPIC_PLASTIC [2,3a,3c] {20} 
*MAT_DAMAGE_1 [0,2,3a,3c] {11} 
*MAT_DAMAGE_2 [0,2,3a,3c] {7} 
*MAT_ELASTIC_VISCOPLASTIC_THERMAL [0,2,3a,3c,5] {20} 
*MAT_MODIFIED_JOHNSON_COOK [0,2,3a,3c,5,8B] {15} 
*MAT_ORTHO_ELASTIC_PLASTIC [2,3a] {15} 
*MAT_JOHNSON_HOLMQUIST_CERAMICS [0,3c,5] {15} 
*MAT_JOHNSON_HOLMQUIST_CONCRETE [0,3c,5] {25} 
*MAT_FINITE_ELASTIC_STRAIN_PLASTICITY [0,3c,5] {22} 
*MAT_TRIP [2,3a] {5} 
*MAT_LAYERED_LINEAR_PLASTICITY [2,3a] {13} 
*MAT_UNIFIED_CREEP [0,2,3a,3c,5] {1} 
*MAT_UNIFIED_CREEP_ORTHO [0,3c,5] {1} 
*MAT_COMPOSITE_LAYUP [2] {30} 
*MAT_COMPOSITE_MATRIX [2] {30} 
*MAT_COMPOSITE_DIRECT [2] {10} 
*MAT_GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM [1D] {62} 
*MAT_GURSON [0,2,3a,3c] {12} 
*MAT_GURSON_JC [0,2] {12} 
*MAT_GURSON_RCDC [0,2] {12} 
*MAT_GENERAL_NONLINEAR_1DOF_DISCRETE_BEAM [1D] {20} 
*MAT_HILL_3R [2,3a] {8} 
*MAT_HILL_3R_3D [0] {28} 
*MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY [0,2,3a,3c,5] {11} 
*MAT_PLASTICITY_COMPRESSION_TENSION [0,1H,2,3a,3c,5,8B] {7} 
*MAT_KINEMATIC_HARDENING_TRANSVERSELY_ANISOTROPIC [0,2,3a,3c] {11} 
*MAT_MODIFIED_HONEYCOMB [0,3c] {20} 
*MAT_ARRUDA_BOYCE_RUBBER [0,3c,5] {49} 
*MAT_HEART_TISSUE [0,3c] {15} 
*MAT_LUNG_TISSUE [0,3c] {49} 
*MAT_SPECIAL_ORTHOTROPIC [2] {35} 
*MAT_ISOTROPIC_SMEARED_CRACK [0,5,8B] {15} 
*MAT_ORTHOTROPIC_SMEARED_CRACK [0] {61} 
*MAT_BARLAT_YLD2000 [2,3a] {9} 
*MAT_VISCOELASTIC_FABRIC [9] 
*MAT_WTM_STM [2,3a] {30} 
*MAT_WTM_STM_PLC [2,3a] {30} 
*MAT_CORUS_VEGTER [2,3a] {5} 
*MAT_COHESIVE_MIXED_MODE [7] {0} 
*MAT_MODIFIED_FORCE_LIMITED [1B] {35} 
*MAT_VACUUM [0,8A] {0}
*MAT_141: 
*MAT_142: 
*MAT_143: 
*MAT_144: 
*MAT_145: 
*MAT_146: 
*MAT_147 
*MAT_147_N: 
*MAT_148: 
*MAT_151: 
*MAT_153: 
*MAT_154: 
*MAT_155: 
*MAT_156: 
*MAT_157: 
*MAT_158: 
*MAT_159: 
*MAT_160: 
*MAT_161: 
*MAT_162: 
*MAT_163 
*MAT_164: 
*MAT_165: 
*MAT_165B: 
*MAT_166: 
*MAT_167: 
*MAT_168: 
*MAT_169: 
*MAT_170: 
*MAT_171: 
*MAT_172: 
*MAT_173: 
*MAT_174: 
*MAT_175: 
*MAT_176: 
*MAT_177: 
*MAT_178: 
*MAT_179: 
*MAT_181: 
*MAT_183: 
*MAT_184: 
*MAT_185: 
*MAT_186: 
*MAT_187: 
*MAT_188: 
*MAT_189: 
*MAT_190: 
*MAT_191: 
*MAT_192: 
*MAT_193: 
*MAT_194: 
*MAT_195: 
*MAT_196: 
*MAT_197: 
*MAT_RATE_SENSITIVE_POLYMER [0,3c,8B] {6} 
*MAT_TRANSVERSELY_ISOTROPIC_CRUSHABLE_FOAM [0,3c] {12} 
*MAT_WOOD_{OPTION} [0,3c,5] {37} 
*MAT_PITZER_CRUSHABLE_FOAM [0,3c,8B] {7} 
*MAT_SCHWER_MURRAY_CAP_MODEL [0,5] {50} 
*MAT_1DOF_GENERALIZED_SPRING [1D] {1} 
*MAT_FHWA_SOIL [0,3c,5,8B] {15} 
*MAT_FHWA_SOIL_NEBRASKA [0,3c,5,8B] {15} 
*MAT_GAS_MIXTURE [0,8A] {14} 
*MAT_EMMI [0,3c,5,8B] {23} 
*MAT_DAMAGE_3 [0,1H,2,3a,3c] 
*MAT_DESHPANDE_FLECK_FOAM [0,3c,8B] {10} 
*MAT_PLASTICITY_COMPRESSION_TENSION_EOS [0,3c,5,8B] {16} 
*MAT_MUSCLE [1T] {0} 
*MAT_ANISOTROPIC_ELASTIC_PLASTIC [0,2,3a] {5} 
*MAT_RATE_SENSITIVE_COMPOSITE_FABRIC [2,3a] {54} 
*MAT_CSCM_{OPTION} [0,3c,5] {22} 
*MAT_ALE_INCOMPRESSIBLE 
*MAT_COMPOSITE_MSC [0] {34} 
*MAT_COMPOSITE_DMG_MSC [0] {40} 
*MAT_MODIFIED_CRUSHABLE_FOAM [0,3c,8B] {10} 
*MAT_BRAIN_LINEAR_VISCOELASTIC [0] {14} 
*MAT_PLASTIC_NONLINEAR_KINEMATIC [0,2,3a,3c,8B] {8} 
*MAT_PLASTIC_NONLINEAR_KINEMATIC_B [0,2] 
*MAT_MOMENT_CURVATURE_BEAM [1B] {54} 
*MAT_MCCORMICK [03c,,8B] {8} 
*MAT_POLYMER [0,3c,8B] {60} 
*MAT_ARUP_ADHESIVE [0] {30} 
*MAT_RESULTANT_ANISOTROPIC [2,3a] {67} 
*MAT_STEEL_CONCENTRIC_BRACE [1B] {35} 
*MAT_CONCRETE_EC2 [1H,2,3a] {64} 
*MAT_MOHR_COULOMB [0,5] {52} 
*MAT_RC_BEAM [1H] {22} 
*MAT_VISCOELASTIC_THERMAL [0,2,3a,3c,5,8B] {86} 
*MAT_QUASILINEAR_VISCOELASTIC [0,2,3a,3c,5,8B] {81} 
*MAT_HILL_FOAM [0,3c] {12} 
*MAT_VISCOELASTIC_HILL_FOAM [0,3c] {92} 
*MAT_LOW_DENSITY_SYNTHETIC_FOAM_{OPTION} [0,3c] {77} 
*MAT_SIMPLIFIED_RUBBER/FOAM_{OPTION} [0,2,3c] {39} 
*MAT_SIMPLIFIED_RUBBER_WITH_DAMAGE [0,2,3c] {44} 
*MAT_COHESIVE_ELASTIC [7] {0} 
*MAT_COHESIVE_TH [7] {0} 
*MAT_COHESIVE_GENERAL [7] {6} 
*MAT_SAMP-1 [0,2,3a,3c] {38} 
*MAT_THERMO_ELASTO_VISCOPLASTIC_CREEP [0,2,3a,3c] {27} 
*MAT_ANISOTROPIC_THERMOELASTIC [0,3c,8B] {21} 
*MAT_FLD_3-PARAMETER_BARLAT [2,3a] {36} 
*MAT_SEISMIC_BEAM [1B] {36} 
*MAT_SOIL_BRICK [0,3c] {96} 
*MAT_DRUCKER_PRAGER [0,3c] {24} 
*MAT_RC_SHEAR_WALL [2,3a] {36} 
*MAT_CONCRETE_BEAM [1H] {5} 
*MAT_GENERAL_SPRING_DISCRETE_BEAM [1D] {25} 
*MAT_SEISMIC_ISOLATOR [1D] {20}
*MAT_JOINTED_ROCK [0] {31} 
*MAT_STEEL_EC3 [1H] {3} 
*MAT_HYSTERETIC_REINFORCEMENT [1H,2] {64} 
*MAT_BOLT_BEAM [1D] {16} 
*MAT_SPR_JLR [1H] {60} 
*MAT_DRY_FABRIC [9] 
*MAT_4A_MICROMEC [0,2,3a,3c] 
*MAT_ELASTIC_PHASE_CHANGE [0] 
*MAT_OPTION_TROPIC_ELASTIC_PHASE_CHANGE [0] 
*MAT_MOONEY-RIVLIN_RUBBER_PHASE_CHANGE [0] 
*MAT_CODAM2 [0,2,3a,3c] 
*MAT_RIGID_DISCRETE [0,2] 
*MAT_ORTHOTROPIC_SIMPLIFIED_DAMAGE [0,3c,5] {17} 
*MAT_TABULATED_JOHNSON_COOK [0,2,3a,3c,,5] {17} 
*MAT_TABULATED_JOHNSON_COOK_GYS [0] {17} 
*MAT_VISCOPLASTIC_MIXED_HARDENING [0,2,3a,3c,5] 
*MAT_KINEMATIC_HARDENING_BARLAT89 [2,3a] 
*MAT_PML_ELASTIC [0] {24} 
*MAT_PML_ACOUSTIC [6] {35} 
*MAT_BIOT_HYSTERETIC [0,2,3a] {30} 
*MAT_CAZACU_BARLAT [2,3a] 
*MAT_VISCOELASTIC_LOOSE_FABRIC [2,3a] 
*MAT_MICROMECHANICS_DRY_FABRIC [2,3a] 
*MAT_SCC_ON_RCC [2,3a] 
*MAT_PML_HYSTERETIC [0] {54} 
*MAT_PERT_PIECEWISE_LINEAR_PLASTICITY [0,1H,2,3,5,8A] 
*MAT_COHESIVE_MIXED_MODE_ELASTOPLASTIC_RATE [7] {0} 
*MAT_JOHNSON_HOLMQUIST_JH1 [0,3c,5] 
*MAT_KINEMATIC_HARDENING_BARLAT2000 [2,3a] 
*MAT_HILL_90 [2,3a] 
*MAT_UHS_STEEL [0,2,3a,3c,5] {35} 
*MAT_PML_{OPTION}TROPIC_ELASTIC [0] {30} 
*MAT_PML_NULL [0] {27} 
*MAT_PHS_BMW [2] {38} 
*MAT_REINFORCED_THERMOPLASTIC [2] 
*MAT_198: 
*MAT_202: 
*MAT_203: 
*MAT_208: 
*MAT_211: 
*MAT_214: 
*MAT_215: 
*MAT_216: 
*MAT_217: 
*MAT_218: 
*MAT_219: 
*MAT_220: 
*MAT_221: 
*MAT_224: 
*MAT_224_GYS: 
*MAT_225: 
*MAT_226: 
*MAT_230: 
*MAT_231: 
*MAT_232: 
*MAT_233: 
*MAT_234: 
*MAT_235: 
*MAT_236: 
*MAT_237: 
*MAT_238: 
*MAT_240: 
*MAT_241: 
*MAT_242: 
*MAT_243: 
*MAT_244: 
*MAT_245: 
*MAT_246: 
*MAT_248: 
*MAT_249: 
*MAT_249_UDFIBER: *MAT_REINFORCED_THERMOPLASTIC_UDFIBER [2] 
*MAT_251: 
*MAT_252: 
*MAT_254: 
*MAT_255: 
*MAT_256: 
*MAT_260A: 
*MAT_260B: 
*MAT_261: 
*MAT_262: 
*MAT_264: 
*MAT_266: 
*MAT_267: 
*MAT_269: 
*MAT_270: 
*MAT_271: 
*MAT_272: 
*MAT_273: 
*MAT_274: 
*MAT_TAILORED_PROPERTIES [2] {6} 
*MAT_TOUGHENED_ADHESIVE_POLYMER [0,7] {10} 
*MAT_GENERALIZED_PHASE_CHANGE [0,2] 
*MAT_PIECEWISE_LINEAR_PLASTIC_THERMAL [0,2,3a,3c] 
*MAT_AMORPHOUS_SOLIDS_FINITE_STRAIN [0]  
*MAT_STOUGHTON_NON_ASSOCIATED_FLOW [0,2] 
*MAT_MOHR_NON_ASSOCIATED_FLOW [0,2] 
*MAT_LAMINATED_FRACTURE_DAIMLER_PINHO [0,2,3a,3c]  
*MAT_LAMINATED_FRACTURE_DAIMLER_CAMANHO [0,2,3a,3c]  
*MAT_TABULATED_JOHNSON_COOK_ORTHO_PLASTICITY [0] 
*MAT_TISSUE_DISPERSED [0]  
*MAT_EIGHT_CHAIN_RUBBER [0,5] 
*MAT_BERGSTROM_BOYCE_RUBBER [0,5] 
*MAT_CWM [0,2,5] 
*MAT_POWDER [0,5] 
*MAT_RHT [0,5]  
*MAT_CONCRETE_DAMAGE_PLASTIC_MODEL [0] 
*MAT_PAPER [0,2]
*MAT_275: 
*MAT_276: 
*MAT_277: 
*MAT_278:  
*MAT_279: 
*MAT_280: 
*MAT_293:  
*MAT_SMOOTH_VISCOELASTIC_VISCOPLASTIC [0] 
*MAT_CHRONOLOGICAL_VISCOELASTIC [2,3a,3c] 
*MAT_ADHESIVE_CURING_VISCOELASTIC [0] 
*MAT_CF_MICROMECHANICS [02] {3} 
*MAT_COHESIVE_PAPER [7] 
*MAT_GLASS [2] {32} 
*MAT_COMPRF [2] {7} 
For the discrete (type 6) beam elements, which are used to model complicated dampers 
and  multi-dimensional  spring-damper  combinations,  the  following  material  types  are 
available: 
*MAT_066: 
*MAT_067: 
*MAT_068: 
*MAT_069: 
*MAT_070: 
*MAT_071: 
*MAT_074: 
*MAT_093: 
*MAT_094: 
*MAT_095: 
*MAT_119: 
*MAT_121: 
*MAT_146: 
*MAT_196: 
*MAT_197: 
*MAT_208: 
*MAT_LINEAR_ELASTIC_DISCRETE_BEAM [1D] 
*MAT_NONLINEAR_ELASTIC_DISCRETE_BEAM [1D] 
*MAT_NONLINEAR_PLASTIC_DISCRETE_BEAM [1D] 
*MAT_SID_DAMPER_DISCRETE_BEAM [1D] 
*MAT_HYDRAULIC_GAS_DAMPER_DISCRETE_BEAM [1D] 
*MAT_CABLE_DISCRETE_BEAM [1D] 
*MAT_ELASTIC_SPRING_DISCRETE_BEAM [1D] 
*MAT_ELASTIC_6DOF_SPRING_DISCRETE_BEAM [1D] 
*MAT_INELASTIC_SPRING_DISCRETE_BEAM [1D] 
*MAT_INELASTIC_6DOF_SPRING_DISCRETE_BEAM [1D] 
*MAT_GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM [1D] 
*MAT_GENERAL_NONLINEAR_1DOF_DISCRETE_BEAM [1D] 
*MAT_1DOF_GENERALIZED_SPRING [1D] 
*MAT_GENERAL_SPRING_DISCRETE_BEAM [1D] 
*MAT_SEISMIC_ISOLATOR [1D] 
*MAT_BOLT_BEAM [1D] 
For the discrete springs and dampers the following material types are available 
*MAT_S01: 
*MAT_S02: 
*MAT_S03: 
*MAT_S04: 
*MAT_S05: 
*MAT_S06: 
*MAT_S07: 
*MAT_S08: 
*MAT_S13: 
*MAT_S14: 
*MAT_S15: 
*MAT_SPRING_ELASTIC 
*MAT_DAMPER_VISCOUS 
*MAT_SPRING_ELASTOPLASTIC 
*MAT_SPRING_NONLINEAR_ELASTIC 
*MAT_DAMPER_NONLINEAR_VISCOUS 
*MAT_SPRING_GENERAL_NONLINEAR 
*MAT_SPRING_MAXWELL 
*MAT_SPRING_INELASTIC 
*MAT_SPRING_TRILINEAR_DEGRADING 
*MAT_SPRING_SQUAT_SHEARWALL 
*MAT_SPRING_MUSCLE 
For ALE solids the following material types are available: 
*MAT_ALE_01: 
*MAT_ALE_02: 
*MAT_ALE_03: 
*MAT_ALE_04: 
*MAT_ALE_05: 
*MAT_ALE_06: 
*MAT_ALE_VACUUM  
*MAT_ALE_GAS_MIXTURE  
*MAT_ALE_VISCOUS  
*MAT_ALE_MIXING_LENGTH 
*MAT_ALE_INCOMPRESSIBLE 
*MAT_ALE_HERSCHEL 
(same as *MAT_140) 
(same as *MAT_148) 
(same as *MAT_009) 
(same as *MAT_149) 
(same as *MAT_160)
For SPH particles the following material type is available: 
*MAT_SPH_01: 
*MAT_SPH_VISCOUS  
(same as *MAT_009) 
For the seatbelts one material is available. 
*MAT_B01: 
*MAT_SEATBELT 
For  thermal  materials  in  a  coupled  structural/thermal  or  thermal  only  analysis,  six 
materials  are  available.    These  materials  are  related  to  the  structural  material  via  the 
*PART card. 
*MAT_T01: 
*MAT_T02: 
*MAT_T03: 
*MAT_T04: 
*MAT_T05: 
*MAT_T07: 
*MAT_T08 
*MAT_T09 
*MAT_T10 
*MAT_T11-T15: 
*MAT_THERMAL_ISOTROPIC 
*MAT_THERMAL_ORTHOTROPIC 
*MAT_THERMAL_ISOTROPIC_TD 
*MAT_THERMAL_ORTHOTROPIC_TD 
*MAT_THERMAL_DISCRETE_BEAM 
*MAT_THERMAL_CWM 
*MAT_THERMAL_ORTHOTROPIC_TD_LC 
*MAT_THERMAL_ISOTROPIC_PHASE_CHANGE 
*MAT_THERMAL_ISOTROPIC_TD_LC 
*MAT_THERMAL_USER_DEFINED DEFINED  
Remarks: 
Curves  and  tables  are  sometimes  defined  for  the  purpose  of  defining  material 
properties.  An example would be a curve of effective stress vs.  effective plastic strain 
defined  using  the  command  *DEFINE_CURVE.    In  general,  the  following  can  be  said 
about curves and tables that are referenced by material models:   
1.  Curves are internally rediscretized using equal increments along the 𝑥-axis.   
2.  Curve data is interpolated between rediscretized data points within the defined 
range of the curve and extrapolated as needed beyond the defined range of the 
curve. 
3.  Extrapolation  is  not  employed  for  table  values  see  the  manual  entries  for  the 
*DEFINE_TABLE_… keywords.
MATERIAL MODEL REFERENCE TABLES 
The  tables  provided  on  the  following  pages  list  the  material  models,  some  of  their 
attributes, and the general classes of physical materials to which the numerical models 
might be applied. 
If  a  material  model,  without  consideration  of  *MAT_ADD_EROSION,  *MAT_ADD_-
THERMAL_EXPANSION, or *MAT_ADD_GENERALIZED_DAMAGE, includes any of 
the following attributes, a “Y” will appear in the respective column of the table: 
SRATE 
FAIL 
EOS 
-  Strain-rate effects 
-  Failure criteria 
-  Equation-of-State  required  for  3D  solids  and  2D 
continuum elements 
THERMAL  -  Thermal effects  
ANISO 
DAM 
TENS 
-  Anisotropic/orthotropic 
-  Damage effects 
-  Tension  handled  differently  than  compression  in 
some manner 
Potential applications of the material models, in terms of classes of physical materials, 
are abbreviated in the table as follows: 
GN  -  General 
CM  -  Composite 
CR  -  Ceramic 
FL 
-  Fluid 
FM  -  Foam 
GL  -  Glass 
HY  -  Hydrodynamic material 
MT  -  Metal 
-  Plastic 
PL 
RB  -  Rubber 
SL 
AD  -  Adhesive or Cohesive material 
BIO  -  Biological material 
CIV  -  Civil Engineering component 
HT  -  Heat Transfer 
F 
-  Soil, concrete, or rock 
-  Fabric
Y 
Y 
Material Number And Description 
Elastic 
Orthotropic Elastic (Anisotropic-solids) 
Plastic Kinematic/Isotropic 
Y  Y 
Elastic Plastic Thermal 
Soil and Foam 
Linear Viscoelastic 
Blatz-Ko Rubber 
High Explosive Burn 
Null Material 
Y 
Y 
Y  Y  Y 
Elastic Plastic Hydro(dynamic) 
Y  Y 
APPS 
GN, 
FL 
CM, 
MT 
CM, 
MT, 
PL 
MT, 
PL 
Y  FM, SL
RB 
RB 
HY 
FL, 
HY 
HY, 
MT 
HY, 
MT 
MT 
Y 
Y 
Y 
Steinberg: Temp.  Dependent 
Elastoplastic 
Isotropic Elastic Plastic 
Isotropic Elastic with Failure 
Soil and Foam with Failure 
Y  Y  Y  Y 
Y 
Y 
Y  MT 
Y  FM, SL
Johnson/Cook Plasticity Model 
Y  Y  Y  Y 
Y  Y 
Pseudo Tensor Geological Model 
Y  Y  Y 
Y  Y 
Oriented Crack (Elastoplastic w/ 
Fracture) 
Y  Y 
Y 
Y 
Power Law Plasticity (Isotropic) 
Y 
Strain Rate Dependent Plasticity 
Y  Y 
Rigid 
Orthotropic Thermal (Elastic) 
Y  Y 
HY, 
MT 
SL 
HY, 
MT, 
PL, CR
MT, 
PL 
MT, 
PL 
GN 
2-10 (EOS) 
LS-DYNA R10.0 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
11 
12 
13 
14 
15 
16 
17 
18 
19
Material Number And Description 
Composite Damage 
Y 
Y 
Temperature Dependent Orthotropic 
Y  Y 
Piecewise Linear Plasticity (Isotropic) 
Y  Y 
Inviscid Two Invariant Geologic Cap 
Y 
Honeycomb 
Y  Y 
Y 
Mooney-Rivlin Rubber 
Resultant Plasticity 
Force Limited Resultant Formulation 
Shape Memory 
Frazer-Nash Rubber 
Laminated Glass (Composite) 
Y 
Barlat Anisotropic Plasticity (YLD96) 
Fabric 
Plastic-Green Naghdi Rate 
Three-Parameter Barlat Plasticity 
Transversely Anisotropic Elastic Plastic 
Y 
Y 
Y 
Y 
Y 
Y  Y 
Y 
Y 
Blatz-Ko Foam 
FLD Transversely Anisotropic 
Nonlinear Orthotropic 
-50 User Defined Materials 
Y  Y  Y  Y  Y  Y  Y 
Y 
Y  Y 
Y 
Bamman (Temp/Rate Dependent 
Plasticity) 
Bamman Damage 
Closed cell foam (Low density 
polyurethane) 
Composite Damage with Chang Failure 
Composite Damage with Tsai-Wu Failure 
Low Density Urethane Foam 
Laminated Composite Fabric 
Y 
Y  Y 
Y 
Y 
Y  Y 
Y 
Y 
Y 
Y 
Y  Y  Y 
Y  Y  Y 
Y 
LS-DYNA R10.0 
Y  Y  Y  CM, F 
2-11 (EOS) 
Y 
Y 
Y 
Y 
Y 
Y 
APPS 
CM 
CM 
MT, 
PL 
SL 
CM, 
FM, SL
RB 
MT 
MT 
RB 
CM, 
GL 
CR, 
MT 
Y 
F 
MT 
MT 
MT 
FM, 
PL 
MT 
CM 
GN 
GN 
MT 
FM 
CM 
CM 
FM 
22 
23 
24 
25 
26 
27 
28 
29 
30 
31 
32 
33 
34 
35 
36 
37 
38 
39 
40 
41 
51 
52 
53 
54 
55
Material Number And Description 
Composite Failure (Plasticity Based) 
Elastic with Viscosity (Viscous Glass) 
Kelvin-Maxwell Viscoelastic 
Viscous Foam (Crash dummy Foam) 
Isotropic Crushable Foam 
Rate Sensitive Powerlaw Plasticity 
Y 
Y 
Y 
Y 
Y 
Y 
Y 
Y 
Y 
APPS 
CM, 
CR 
GL 
FM 
FM 
FM 
MT 
Zerilli-Armstrong (Rate/Temp Plasticity)  Y 
Y  Y 
Y  MT 
Linear Elastic Discrete Beam 
Nonlinear Elastic Discrete Beam 
Y 
Y 
Nonlinear Plastic Discrete Beam 
Y  Y 
SID Damper Discrete Beam 
Hydraulic Gas Damper Discrete Beam 
Cable Discrete Beam (Elastic) 
Y 
Y 
Y 
Y 
Y 
Y 
Y  Cables 
Concrete Damage (incl.  Release III) 
Y  Y  Y 
Y  Y 
Low Density Viscous Foam 
Elastic Spring Discrete Beam 
Bilkhu/Dubois Foam 
General Viscoelastic (Maxwell Model) 
Hyperelastic and Ogden Rubber 
Soil Concrete 
Hysteretic Soil (Elasto-Perfectly Plastic) 
Ramberg-Osgood 
Plasticity with Damage 
Plasticity with Damage Ortho 
Fu Chang Foam 
Winfrith Concrete 
Orthotropic Viscoelastic 
Cellular Rubber 
MTS 
Plasticity Polymer 
Y  Y 
Y  Y 
Y 
Y 
Y 
Y 
Y  Y 
Y  Y 
Y  Y 
Y 
Y 
Y 
Y 
Y 
SL 
FM 
FM 
RB 
RB 
SL 
SL 
SL 
MT, 
PL 
Y 
Y 
Y 
Y 
Y 
Y 
Y  Y 
Y 
Y 
Y  Y 
Y 
Y  Y 
Y  Y 
FM 
Y  FM, SL
RB 
RB 
MT 
PL 
Y 
Y 
LS-DYNA R10.0 
59 
60 
61 
62 
63 
64 
65 
66 
67 
68 
69 
70 
71 
72 
73 
74 
75 
76 
77 
78 
79 
80 
81 
82 
83 
84 
86 
87 
88
Material Number And Description 
90 
91 
92 
93 
94 
95 
96 
97 
98 
99 
100 
101 
Acoustic 
Soft Tissue 
Soft Tissue (viscous) 
Elastic 6DOF Spring Discrete Beam 
Inelastic Spring Discrete Beam 
Inelastic 6DOF Spring Discrete Beam 
Brittle Damage 
General Joint Discrete Beam 
Simplified Johnson Cook 
Simpl.  Johnson Cook Orthotropic 
Damage 
Spotweld 
GE Plastic Strain Rate 
Y  Y 
Y  Y 
Y  Y 
Y  Y 
Y  Y 
Y  Y 
Y  Y 
Y  Y 
Y  Y 
102(_T) 
Inv.  Hyperbolic Sin (Thermal) 
Y 
Y 
103 
103P 
Anisotropic Viscoplastic 
Anisotropic Plastic 
Y  Y 
Y  Y 
Y  Y 
Y 
Y  Y 
Y  Y 
Y  Y 
Y 
Y 
Y 
Y 
Damage 1 
Damage 2 
Elastic Viscoplastic Thermal 
Modified Johnson Cook 
Ortho Elastic Plastic 
Johnson Holmquist Ceramics 
Johnson Holmquist Concrete 
Finite Elastic Strain Plasticity 
104 
105 
106 
107 
108 
110 
111 
112 
113 
114 
115 
115_O 
116 
Unified Creep 
Unified Creep Ortho 
Composite Layup 
Transformation Induced Plasticity (TRIP) 
Layered Linear Plasticity 
Y  Y 
APPS 
FL 
BIO 
Y 
Y 
Y 
Y 
Y 
Y 
Y 
Y 
Y  Y  Y 
SL 
Y  Y 
MT 
MT 
Y  Y  MT 
Y 
Y 
Y 
Y  Y 
Y 
Y 
Y 
Y  Y 
Y  Y 
Y 
Y 
PL 
MT, 
PL 
MT 
MT 
MT 
MT 
PL 
MT 
CR, 
GL 
SL 
PL 
MT 
MT, 
PL, 
CM 
GN 
GN 
CM
Material Number And Description 
117 
118 
119 
120 
121 
122 
Composite Matrix 
Composite Direct 
General Nonlinear 6DOF Discrete Beam 
Gurson 
General Nonlinear 1DOF Discrete Beam 
Hill 3RC 
122_3D  Hill 3R 3D 
Modified Piecewise Linear Plasticity 
Plasticity Compression Tension 
Kinematic Hardening Transversely 
Aniso. 
Y  Y 
Y  Y 
Y  Y 
Y  Y 
Y  Y 
Y 
Y 
Y 
Y 
Y 
Y 
123 
124 
125 
126 
127 
128 
129 
130 
131 
132 
133 
134 
135 
136 
138 
139 
140 
141 
142 
143 
Modified Honeycomb 
Y  Y 
Y  Y  Y 
Arruda Boyce Rubber 
Heart Tissue 
Lung Tissue 
Special Orthotropic 
Isotropic Smeared Crack 
Orthotropic Smeared Crack 
Barlat YLD2000 
Viscoelastic Fabric 
Y 
Y 
Y 
Y 
Y 
Y 
Y 
Y 
Y  Y 
Y  Y 
Y 
Y  Y 
Weak and Strong Texture Model 
Y  Y 
Corus Vegter 
Cohesive Mixed Mode 
Modified Force Limited 
Vacuum 
Y 
Y 
Y 
Y  Y  Y 
Y  Y 
Rate Sensitive Polymer 
Y 
Transversely Isotropic Crushable Foam 
PL 
FM 
Y 
Wood 
Y  Y 
Y  Y  Y  Wood 
2-14 (EOS) 
LS-DYNA R10.0 
APPS 
CM 
CM 
Y 
Y  Y  MT 
Y 
Y 
MT 
MT, 
CM 
MT, 
PL 
MT, 
PL 
MT 
CM, 
FM, SL
RB 
BIO 
BIO 
MT, 
CM 
MT, 
CM 
MT 
MT
Y 
Y  Y 
Y 
Y 
Y 
Y 
Y 
Y  Y 
Y  Y 
Y  Y 
Y  Y 
Y  Y  Y 
Material Number And Description 
144 
145 
146 
147 
Pitzer Crushable Foam 
Schwer Murray Cap Model 
1DOF Generalized Spring 
FWHA Soil 
147N 
FHWA Soil Nebraska 
Gas Mixture 
Evolving Microstructural Model of 
Inelast. 
148 
151 
153 
154 
155 
156 
157 
158 
159 
160 
Damage 3 
Deshpande Fleck Foam 
Y  Y 
Y 
Plasticity Compression Tension EOS 
Y  Y  Y 
Muscle 
Anisotropic Elastic Plastic 
Rate-Sensitive Composite Fabric 
CSCM 
ALE incompressible 
Y 
Y  Y 
Y  Y 
Y 
Y 
Y 
Y 
Y  Y  Y 
Y  Y 
161,162 
Composite MSC (Dmg) 
Y  Y 
Y  Y  Y 
163 
164 
165 
165B 
166 
167 
168 
169 
170 
171 
172 
173 
174 
Modified Crushable Foam 
Brain Linear Viscoelastic 
Plastic Nonlinear Kinematic 
Plastic Nonlinear Kinematic_B 
Moment Curvature Beam 
McCormick 
Polymer 
Arup Adhesive 
Resultant Anisotropic 
Steel Concentric Brace 
Concrete EC2 
Mohr Coulomb 
RC Beam 
Y 
Y 
Y 
Y  Y 
Y 
Y  Y 
Y 
Y 
Y 
Y 
Y 
Y 
Y 
Y  Y 
Y 
Y 
Y  Y 
Y 
Y 
Y 
APPS 
FM 
SL 
SL 
SL 
FL 
MT 
MT, 
PL 
FM 
Ice 
BIO 
MT, 
CM 
CM 
SL 
CM 
FM 
BIO 
MT 
MT 
CIV 
MT 
PL 
AD 
PL 
CIV 
SL, 
MT 
SL 
SL
Y 
Y 
Material Number And Description 
Viscoelastic Thermal 
Quasilinear Viscoelastic 
Hill Foam 
Viscoelastic Hill Foam (Ortho) 
Low Density Synthetic Foam 
Simplified Rubber/Foam 
Simplified Rubber with Damage 
Cohesive Elastic 
Cohesive TH 
Cohesive General 
Semi-Analytical Model for Polymers – 1 
Thermo Elasto Viscoelastic Creep 
Anisotropic Thermoelastic 
Y  Y 
Y 
Y  Y 
Y  Y 
Y 
Y 
Y 
Y 
Y  Y 
Y 
Y 
Y  Y 
Y 
Y 
Y  Y  Y 
Y  Y 
Y  Y 
Y 
Y  Y  Y 
Y  Y  Y 
Y  Y 
APPS 
RB 
BIO 
FM 
FM 
FM 
RB, 
FM 
RB 
AD 
AD 
AD 
PL 
MT 
Y 
Y  Y 
Flow limit diagram 3-Parameter  Barlat 
Y 
Seismic Beam 
Soil Brick 
Drucker Prager 
RC Shear Wall 
Concrete Beam 
General Spring Discrete Beam 
Seismic Isolator 
Jointed Rock 
Steel EC3 
Hysteretic Reinforcement 
Bolt Beam 
SPR JLR 
Dry Fabric 
4A Micromec 
Elastic Phase Change 
Orthotropic Elastic Phase Change 
Mooney Rivlin Rubber Phase Change 
Y 
Y  Y 
Y 
Y  Y 
Y 
Y 
Y 
Y  Y 
Y  Y 
Y  Y 
Y 
Y 
Y 
Y 
Y  MT 
Y 
CIV 
Y 
Y  Y 
Y  Y 
Y 
Y 
Y 
Y  Y 
SL 
SL 
CIV 
CIV 
CIV 
SL 
CIV 
CV 
Y  Y  MT 
MT 
Y  Y  Y 
Y  Y 
  CM,PL
Y 
GN 
GN 
RB 
Y 
LS-DYNA R10.0 
175 
176 
177 
178 
179 
181 
183 
184 
185 
186 
187 
188 
189 
190 
191 
192 
193 
194 
195 
196 
197 
198 
202 
203 
208 
211 
214 
215 
216 
217
Material Number And Description 
CODAM2 
Rigid Discrete 
Orthotropic Simplified Damage 
Y 
Y 
APPS 
Y  Y  Y 
CM 
Y  Y  Y 
Tabulated Johnson Cook 
Y  Y  Y  Y 
Y  Y 
219 
220 
221 
224 
224_GYS  Tabulated Johnson Cook GYS 
Y  Y  Y  Y 
Y  Y 
225 
226 
230 
231 
232 
233 
234 
235 
236 
237 
238 
240 
241 
242 
243 
244 
245 
246 
248 
249 
Viscoplastic Mixed Hardening 
Y  Y 
Kinematic hardening Barlat 89 
Elastic Perfectly Matched Layer (PML) 
Acoustic PML 
Biot Linear Hysteretic Material 
Cazacu Barlat 
Viscoelastic Loose Fabric 
Micromechanic Dry Fabric 
Ceramic Matrix 
Biot Hysteretic PML 
Piecewise linear plasticity (PERT) 
Cohesive mixed mode 
Johnson Holmquist JH1 
Kinematic hardening Barlat 2000 
Hill 90 
UHS Steel 
Orthotropic/anisotropic PML 
Null material PML 
PHS BMW 
Reinforced Thermoplastic 
Y 
Y 
Y  Y 
Y 
Y 
Y  Y 
Y  Y 
Y  Y 
Y 
Y 
Y 
Y 
LS-DYNA R10.0 
Y 
Y 
Y 
Y 
Y 
Y  Y  Y 
Y  Y 
Y 
Y  Y 
Y 
Y  Y 
Y  Y 
Y 
Y  MT 
Y 
Y 
Y 
CM 
HY, 
MT, 
PL 
HY, 
MT, 
PL 
MT, 
PL 
MT 
SL 
FL 
SL 
Fabric 
Fabric 
CM, 
CR 
SL 
MT, 
PL 
AD 
CR, 
GL 
MT 
MT 
MT 
SL 
FL 
MT
Material Number And Description 
APPS 
249_ 
UDfiber 
Reinforced Thermoplastic UDfiber 
Y  Y 
Y  CM, F 
251 
252 
254 
255 
256 
260A 
260B 
261 
262 
264 
266 
267 
269 
270 
271 
272 
273 
274 
275 
276 
277 
278 
279 
280 
293 
A01 
A02 
A03 
Tailored Properties 
Y  Y 
Toughened Adhesive Polymer 
Y  Y 
Y  Y  Y  Y 
Generalized Phase Change 
Piecewise linear plastic thermal 
Amorphous solid (finite strain) 
Stoughton non-associated flow 
Y 
Y 
Y 
Y  Y 
Y 
Y 
Y  MT 
Y 
Y 
Mohr non-associated flow 
Y  Y 
Y  Y  Y 
Laminated Fracture Daimler Pinho 
Laminated Fracture Daimler Camanho 
Y 
Y 
Y  Y  Y 
Y  Y  Y 
Tabulated Johnson Cook Orthotorpic 
Plasticity 
Y  Y  Y  Y  Y  Y  Y 
MT, 
PL 
AD 
MT 
GL 
MT 
MT 
CM 
CM 
HY, 
MT, 
PL 
BIO 
Dispersed tissue 
Eight chain rubber 
Bergström Boyce rubber 
Welding material 
Powder compaction 
RHT concrete model 
Concrete damage plastic 
Paper 
Smooth viscoelastic viscoplastic 
Chronological viscoelastic 
Adhesive curing viscoelastic 
CF Micromechanics 
Cohesive Paper 
Glass 
COMPRF 
ALE Vacuum 
ALE Gas Mixture 
ALE Viscous 
Y 
Y 
Y  Y 
Y  Y 
Y 
Y 
Y 
Y 
Y 
Y 
Y 
Y 
Y 
RB, PL 
RB 
  MT,PL 
Y  CR,SL 
Y  Y  SL,CIV
Y  Y 
SL 
Y  CM,PL
  MT,PL 
RB 
PL,RB 
Y  Y 
Y  Y 
Y 
Y 
Y 
Y  Y  Y 
Y 
Y 
Y 
Y 
Y 
CM 
AD 
GL 
CM 
FL 
FL 
FL
APPS 
Material Number And Description 
A04 
A05 
A06 
ALE Mixing Length 
ALE Incompressible 
ALE Herschel 
SPH01 
SPH Viscous 
S1 
S2 
S3 
S4 
S5 
S6 
S7 
S8 
S13 
S14 
S15 
B1 
T01 
T02 
T03 
T04 
T05 
T07 
T08 
T09 
T10 
T11 
Y 
Y 
Y 
Y 
Y 
Spring Elastic (Linear) 
Damper Viscous (Linear) 
Spring Elastoplastic (Isotropic) 
Spring Nonlinear Elastic 
Damper Nonlinear Viscous 
Spring General Nonlinear 
Spring Maxwell (3-Parameter 
Viscoelastic) 
Spring Inelastic (Tension or 
Compression) 
Spring Trilinear Degrading 
Spring Squat Shearwall 
Spring Muscle 
Seatbelt 
Thermal Isotropic 
Thermal Orthotropic 
Thermal Isotropic (Temp Dependent) 
Thermal Orthotropic (Temp Dependent) 
Thermal Discrete Beam 
Thermal CWM (Welding) 
Thermal Orthotropic(Temp dep-load 
curve) 
Thermal Isotropic (Phase Change) 
Thermal Isotropic (Temp dep-load curve) 
Thermal User Defined 
Y 
Y 
Y 
Y 
Y 
Y 
Y  Y 
Y 
Y  Y 
Y 
Y 
Y  Y 
Y 
Y 
Y 
Y 
Y 
Y 
Y 
Y 
Y 
Y 
Y 
FL 
FL 
FL 
FL 
CIV 
CIV 
BIO 
HT 
HT 
HT 
HT 
HT 
HT 
HT 
HT 
HT 
HT
ALPHABETIZED MATERIALS LIST 
Alphabetized Materials List 
Material Keyword 
Number 
*EOS 
*EOS_GASKET 
*EOS_GRUNEISEN 
*EOS_IDEAL_GAS 
*EOS_IGNITION_AND_GROWTH_OF_REACTION_IN_HE 
*EOS_JWL 
*EOS_JWLB 
*EOS_LINEAR_POLYNOMIAL 
*EOS_LINEAR_POLYNOMIAL_WITH_ENERGY_LEAK 
*EOS_MIE_GRUNEISEN 
*EOS_PROPELLANT_DEFLAGRATION 
*EOS_RATIO_OF_POLYNOMIALS 
*EOS_SACK_TUESDAY 
*EOS_TABULATED 
*EOS_TABULATED_COMPACTION 
*EOS_TENSOR_PORE_COLLAPSE 
*EOS_USER_DEFINED 
*MAT_{OPTION}TROPIC_ELASTIC  
*MAT_1DOF_GENERALIZED_SPRING  
*MAT_3-PARAMETER_BARLAT  
*MAT_4A_MICROMEC 
*MAT_ACOUSTIC  
*MAT_ADD_AIRBAG_POROSITY_LEAKAGE 
*MAT_ADD_COHESIVE 
*MAT_ADD_EROSION 
*MAT_ADD_FATIGUE 
*MAT_ADD_GENERALIZED_DAMAGE 
*MAT_002 
*MAT_146 
*MAT_036 
*MAT_215 
*MAT_090
ALPHABETIZED MATERIALS LIST  
Material Keyword 
Number 
*MAT_ADD_PERMEABILITY 
*MAT_ADD_PORE_AIR 
*MAT_ADD_THERMAL_EXPANSION 
*MAT_ADHESIVE_CURING_VISCOELASTIC 
*MAT_ALE_GAS_MIXTURE 
*MAT_ALE_HERSCHEL 
*MAT_ALE_INCOMPRESSIBLE 
*MAT_ALE_MIXING_LENGTH 
*MAT_ALE_VACUUM 
*MAT_ALE_VISCOUS 
*MAT_AMORPHOUS_SOLIDS_FINITE_STRAIN   
*MAT_ANISOTROPIC_ELASTIC 
*MAT_ANISOTROPIC_ELASTIC_PLASTIC  
*MAT_ANISOTROPIC_PLASTIC  
*MAT_ANISOTROPIC_THERMOELASTIC 
*MAT_ANISOTROPIC_VISCOPLASTIC  
*MAT_ARRUDA_BOYCE_RUBBER  
*MAT_ARUP_ADHESIVE  
*MAT_BAMMAN  
*MAT_BAMMAN_DAMAGE  
*MAT_BARLAT_ANISOTROPIC_PLASTICITY  
*MAT_BARLAT_YLD2000  
*MAT_BARLAT_YLD96 
*MAT_BERGSTROM_BOYCE_RUBBER  
*MAT_BILKHU/DUBOIS_FOAM  
*MAT_BIOT_HYSTERETIC  
*MAT_BLATZ-KO_FOAM  
*MAT_BLATZ-KO_RUBBER  
*MAT_BOLT_BEAM 
*MAT_BRAIN_LINEAR_VISCOELASTIC  
*MAT_277 
*MAT_ALE_02 
*MAT_ALE_06 
*MAT_160 
*MAT_ALE_04 
*MAT_ALE_01 
*MAT_ALE_03 
*MAT_256 
*MAT_002_ANISO
*MAT_157 
*MAT_103_P 
*MAT_189 
*MAT_103 
*MAT_127 
*MAT_169 
*MAT_051 
*MAT_052 
*MAT_033 
*MAT_133 
*MAT_033_96 
*MAT_269 
*MAT_075 
*MAT_232 
*MAT_038 
*MAT_007 
*MAT_208 
*MAT_164
ALPHABETIZED MATERIALS LIST 
Material Keyword 
Number 
*MAT_BRITTLE_DAMAGE  
*MAT_CABLE_DISCRETE_BEAM  
*MAT_CAZACU_BARLAT  
*MAT_CELLULAR_RUBBER  
*MAT_CF_MICROMECHANICS 
*MAT_CHRONOLOGICAL_VISCOELASTIC  
*MAT_CLOSED_CELL_FOAM  
*MAT_CODAM2  
*MAT_COHESIVE_ELASTIC  
*MAT_COHESIVE_GENERAL  
*MAT_COHESIVE_MIXED_MODE  
*MAT_COHESIVE_MIXED_MODE_ELASTOPLASTIC_RATE  
*MAT_COHESIVE_PAPER 
*MAT_COHESIVE_TH  
*MAT_COMPOSITE_DAMAGE  
*MAT_COMPOSITE_DIRECT 
*MAT_COMPOSITE_DMG_MSC  
*MAT_COMPOSITE_FAILURE_{OPTION}_MODEL 
*MAT_COMPOSITE_LAYUP  
*MAT_COMPOSITE_MATRIX  
*MAT_COMPOSITE_MSC  
*MAT_COMPRF 
*MAT_CONCRETE_BEAM  
*MAT_CONCRETE_DAMAGE  
*MAT_CONCRETE_DAMAGE_PLASTIC_MODEL 
*MAT_CONCRETE_DAMAGE_REL3  
*MAT_CONCRETE_EC2  
*MAT_CORUS_VEGTER  
*MAT_CRUSHABLE_FOAM  
*MAT_CSCM_{OPTION} 
*MAT_096 
*MAT_071 
*MAT_233 
*MAT_087 
*MAT_278 
*MAT_276 
*MAT_053 
*MAT_219 
*MAT_184 
*MAT_186 
*MAT_138 
*MAT_240 
*MAT_279 
*MAT_185 
*MAT_022 
*MAT_118 
*MAT_162 
*MAT_059 
*MAT_116 
*MAT_117 
*MAT_161 
*MAT_293 
*MAT_195 
*MAT_072 
*MAT_273 
*MAT_072R3 
*MAT_172 
*MAT_136 
*MAT_063 
*MAT_159
ALPHABETIZED MATERIALS LIST  
Material Keyword 
Number 
*MAT_CWM  
*MAT_DAMAGE_1  
*MAT_DAMAGE_2  
*MAT_DAMAGE_3  
*MAT_DAMPER_NONLINEAR_VISCOUS 
*MAT_DAMPER_VISCOUS 
*MAT_DESHPANDE_FLECK_FOAM  
*MAT_DRUCKER_PRAGER  
*MAT_DRY_FABRIC  
*MAT_EIGHT_CHAIN_RUBBER  
*MAT_ELASTIC  
*MAT_ELASTIC_6DOF_SPRING_DISCRETE_BEAM  
*MAT_ELASTIC_FLUID  
*MAT_ELASTIC_PHASE_CHANGE 
*MAT_ELASTIC_PLASTIC_HYDRO_{OPTION}  
*MAT_ELASTIC_PLASTIC_THERMAL  
*MAT_ELASTIC_SPRING_DISCRETE_BEAM 
*MAT_ELASTIC_VISCOPLASTIC_THERMAL  
*MAT_ELASTIC_WITH_VISCOSITY  
*MAT_ELASTIC_WITH_VISCOSITY_CURVE  
*MAT_EMMI  
*MAT_ENHANCED_COMPOSITE_DAMAGE  
*MAT_EXTENDED_3-PARAMETER_BARLAT 
*MAT_FABRIC  
*MAT_FABRIC_MAP 
*MAT_FHWA_SOIL  
*MAT_FHWA_SOIL_NEBRASKA  
*MAT_FINITE_ELASTIC_STRAIN_PLASTICITY  
*MAT_FLD_3-PARAMETER_BARLAT  
*MAT_FLD_TRANSVERSELY_ANISOTROPIC  
*MAT_270 
*MAT_104 
*MAT_105 
*MAT_153 
*MAT_S05 
*MAT_S02 
*MAT_154 
*MAT_193 
*MAT_214 
*MAT_267 
*MAT_001 
*MAT_093 
*MAT_001_FLUID 
*MAT_216 
*MAT_010 
*MAT_004 
*MAT_074 
*MAT_106 
*MAT_060 
*MAT_060C 
*MAT_151 
*MAT_054-055 
*MAT_036E 
*MAT_034 
*MAT_034M 
*MAT_147 
*MAT_147_N 
*MAT_112 
*MAT_190 
*MAT_039
ALPHABETIZED MATERIALS LIST 
Material Keyword 
Number 
*MAT_FORCE_LIMITED  
*MAT_FRAZER_NASH_RUBBER_MODEL  
*MAT_FU_CHANG_FOAM  
*MAT_GAS_MIXTURE  
*MAT_GENERAL_JOINT_DISCRETE_BEAM  
*MAT_GENERAL_NONLINEAR_1DOF_DISCRETE_BEAM  
*MAT_GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM  
*MAT_GENERAL_SPRING_DISCRETE_BEAM  
*MAT_GENERAL_VISCOELASTIC  
*MAT_GENERALIZED_PHASE_CHANGE 
*MAT_GEOLOGIC_CAP_MODEL  
*MAT_GEPLASTIC_SRATE_2000a  
*MAT_GLASS 
*MAT_GURSON  
*MAT_GURSON_JC  
*MAT_GURSON_RCDC  
*MAT_HEART_TISSUE  
*MAT_HIGH_EXPLOSIVE_BURN  
*MAT_HILL_3R  
*MAT_HILL_3R_3D 
*MAT_HILL_90 
*MAT_HILL_FOAM  
*MAT_HONEYCOMB 
*MAT_HYDRAULIC_GAS_DAMPER_DISCRETE_BEAM  
*MAT_HYPERELASTIC_RUBBER  
*MAT_HYSTERETIC_REINFORCEMENT 
*MAT_HYSTERETIC_SOIL  
*MAT_INELASTC_6DOF_SPRING_DISCRETE_BEAM  
*MAT_INELASTIC_6DOF_SPRING_DISCRETE_BEAM 
*MAT_INELASTIC_SPRING_DISCRETE_BEAM 
*MAT_029 
*MAT_031 
*MAT_083 
*MAT_148 
*MAT_097 
*MAT_121 
*MAT_119 
*MAT_196 
*MAT_076 
*MAT_254 
*MAT_025 
*MAT_101 
*MAT_280 
*MAT_120 
*MAT_120_JC 
*MAT_120_RCDC 
*MAT_128 
*MAT_008 
*MAT_122 
*MAT_122_3D 
*MAT_243 
*MAT_177 
*MAT_026 
*MAT_070 
*MAT_077_H 
*MAT_203 
*MAT_079 
*MAT_095 
*MAT_095 
*MAT_094
ALPHABETIZED MATERIALS LIST  
Material Keyword 
*MAT_INV_HYPERBOLIC_SIN(_THERMAL) 
*MAT_ISOTROPIC_ELASTIC_FAILURE  
*MAT_ISOTROPIC_ELASTIC_PLASTIC  
*MAT_ISOTROPIC_SMEARED_CRACK  
*MAT_JOHNSON_COOK 
*MAT_JOHNSON_HOLMQUIST_CERAMICS  
*MAT_JOHNSON_HOLMQUIST_CONCRETE  
*MAT_JOHNSON_HOLMQUIST_JH1 
*MAT_JOINTED_ROCK 
*MAT_KELVIN-MAXWELL_VISCOELASTIC  
*MAT_KINEMATIC_HARDENING_BARLAT2000  
*MAT_KINEMATIC_HARDENING_BARLAT89  
Number 
*MAT_102(_T) 
*MAT_013 
*MAT_012 
*MAT_131 
*MAT_015 
*MAT_110 
*MAT_111 
*MAT_241 
*MAT_198 
*MAT_061 
*MAT_242 
*MAT_226 
*MAT_KINEMATIC_HARDENING_TRANSVERSELY_ANISOTROPIC  *MAT_125 
*MAT_LAMINATED_COMPOSITE_FABRIC 
*MAT_LAMINATED_FRACTURE_DAIMLER_CAMANHO 
*MAT_LAMINATED_FRACTURE_DAIMLER_PINHO 
*MAT_LAMINATED_GLASS 
*MAT_LAYERED_LINEAR_PLASTICITY 
*MAT_LINEAR_ELASTIC_DISCRETE_BEAM 
*MAT_LOW_DENSITY_FOAM 
*MAT_LOW_DENSITY_SYNTHETIC_FOAM_{OPTION} 
*MAT_LOW_DENSITY_VISCOUS_FOAM 
*MAT_LUNG_TISSUE 
*MAT_MCCORMICK 
*MAT_MICROMECHANICS_DRY_FABRIC 
*MAT_MODIFIED_CRUSHABLE_FOAM 
*MAT_MODIFIED_FORCE_LIMITED 
*MAT_MODIFIED_HONEYCOMB 
*MAT_MODIFIED_JOHNSON_COOK 
*MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY 
*MAT_058 
*MAT_262 
*MAT_261 
*MAT_032 
*MAT_114 
*MAT_066 
*MAT_057 
*MAT_179 
*MAT_073 
*MAT_129 
*MAT_167 
*MAT_235 
*MAT_163 
*MAT_139 
*MAT_126 
*MAT_107 
*MAT_123
ALPHABETIZED MATERIALS LIST 
Material Keyword 
*MAT_MODIFIED_ZERILLI_ARMSTRONG 
*MAT_MOHR_COULOMB 
*MAT_MOHR_NON_ASSOCIATED_FLOW 
*MAT_MOMENT_CURVATURE_BEAM 
*MAT_MOONEY-RIVLIN_RUBBER 
*MAT_MOONEY-RIVLIN_RUBBER_PHASE_CHANGE 
*MAT_MTS 
*MAT_MUSCLE 
*MAT_NONLINEAR_ELASTIC_DISCRETE_BEAM 
*MAT_NONLINEAR_ORTHOTROPIC 
*MAT_NONLINEAR_PLASTIC_DISCRETE_BEAM 
*MAT_NONLOCAL 
*MAT_NULL 
*MAT_OGDEN_RUBBER 
*MAT_OPTION_TROPIC_ELASTIC 
*MAT_OPTION_TROPIC_ELASTIC_PHASE_CHANGE 
*MAT_ORIENTED_CRACK 
*MAT_ORTHO_ELASTIC_PLASTIC 
*MAT_ORTHOTROPIC_SIMPLIFIED_DAMAGE 
*MAT_ORTHOTROPIC_SMEARED_CRACK 
*MAT_ORTHOTROPIC_THERMAL 
*MAT_ORTHOTROPIC_VISCOELASTIC 
*MAT_PAPER 
*MAT_PERT_PIECEWISE_LINEAR_PLASTICITY 
*MAT_PHS_BMW 
*MAT_PIECEWISE_LINEAR_PLASTIC_THERMAL 
*MAT_PIECEWISE_LINEAR_PLASTICITY 
*MAT_PITZER_CRUSHABLE_FOAM 
*MAT_PLASTIC_GREEN-NAGHDI_RATE 
*MAT_PLASTIC_KINEMATIC 
Number 
*MAT_065 
*MAT_173 
*MAT_260B 
*MAT_166 
*MAT_027 
*MAT_218 
*MAT_088 
*MAT_156 
*MAT_067 
*MAT_040 
*MAT_068 
*MAT_009 
*MAT_077_O 
*MAT_002 
*MAT_217 
*MAT_017 
*MAT_108 
*MAT_221 
*MAT_132 
*MAT_021 
*MAT_086 
*MAT_274 
*MAT_238 
*MAT_248 
*MAT_255 
*MAT_024 
*MAT_144 
*MAT_035 
*MAT_003
ALPHABETIZED MATERIALS LIST  
Material Keyword 
Number 
*MAT_PLASTIC_NONLINEAR_KINEMATIC 
*MAT_PLASTIC_NONLINEAR_KINEMATIC_B 
*MAT_PLASTICITY_COMPRESSION_TENSION 
*MAT_PLASTICITY_COMPRESSION_TENSION_EOS 
*MAT_PLASTICITY_POLYMER 
*MAT_PLASTICITY_WITH_DAMAGE 
*MAT_165 
*MAT_165B 
*MAT_124 
*MAT_155 
*MAT_089 
*MAT_081 
*MAT_PLASTICITY_WITH_DAMAGE_ORTHO(_RCDC) 
*MAT_082(_RCDC) 
*MAT_PML_{OPTION}TROPIC_ELASTIC 
*MAT_PML_ACOUSTIC 
*MAT_PML_ELASTIC 
*MAT_PML_ELASTIC_FLUID 
*MAT_PML_HYSTERETIC 
*MAT_PML_NULL 
*MAT_POLYMER 
*MAT_POWDER 
*MAT_POWER_LAW_PLASTICITY 
*MAT_PSEUDO_TENSOR 
*MAT_QUASILINEAR_VISCOELASTIC 
*MAT_RAMBERG-OSGOOD 
*MAT_RATE_SENSITIVE_COMPOSITE_FABRIC 
*MAT_RATE_SENSITIVE_POLYMER 
*MAT_RATE_SENSITIVE_POWERLAW_PLASTICITY 
*MAT_RC_BEAM 
*MAT_RC_SHEAR_WALL  
*MAT_REINFORCED_THERMOPLASTIC 
*MAT_REINFORCED_THERMOPLASTIC_UDFIBER 
*MAT_RESULTANT_ANISOTROPIC 
*MAT_RESULTANT_PLASTICITY 
*MAT_RHT 
LS-DYNA R10.0 
*MAT_245 
*MAT_231 
*MAT_230 
*MAT_230 
*MAT_237 
*MAT_246 
*MAT_168 
*MAT_271 
*MAT_018 
*MAT_016 
*MAT_176 
*MAT_080 
*MAT_158 
*MAT_141 
*MAT_064 
*MAT_174 
*MAT_194 
*MAT_249 
*MAT_249_ 
 UDFIBER 
*MAT_170 
*MAT_028
ALPHABETIZED MATERIALS LIST 
Material Keyword 
Number 
*MAT_RIGID 
*MAT_RIGID_DISCRETE 
*MAT_SAMP-1 
*MAT_SCC_ON_RCC 
*MAT_SCHWER_MURRAY_CAP_MODEL 
*MAT_SEATBELT 
*MAT_SEISMIC_BEAM 
*MAT_SEISMIC_ISOLATOR 
*MAT_SHAPE_MEMORY 
*MAT_SID_DAMPER_DISCRETE_BEAM 
*MAT_SIMPLIFIED_JOHNSON_COOK 
*MAT_020 
*MAT_220 
*MAT_187 
*MAT_236 
*MAT_145 
*MAT_B01 
*MAT_191 
*MAT_197 
*MAT_030 
*MAT_069 
*MAT_098 
*MAT_SIMPLIFIED_JOHNSON_COOK_ORTHOTROPIC_DAMAGE  
*MAT_099 
*MAT_SIMPLIFIED_RUBBER/FOAM_{OPTION} 
*MAT_SIMPLIFIED_RUBBER_WITH_DAMAGE 
*MAT_SMOOTH_VISCOELASTIC_VISCOPLASTIC 
*MAT_SOFT_TISSUE 
*MAT_SOFT_TISSUE_VISCO 
*MAT_SOIL_AND_FOAM 
*MAT_SOIL_AND_FOAM_FAILURE 
*MAT_SOIL_BRICK  
*MAT_SOIL_CONCRETE 
*MAT_SPECIAL_ORTHOTROPIC 
*MAT_SPH_VISCOUS 
*MAT_SPOTWELD_{OPTION} 
*MAT_SPOTWELD_DAIMLERCHRYSLER 
*MAT_SPR_JLR 
*MAT_SPRING_ELASTIC 
*MAT_SPRING_ELASTOPLASTIC 
*MAT_SPRING_GENERAL_NONLINEAR 
*MAT_SPRING_INELASTIC 
*MAT_181 
*MAT_183 
*MAT_275 
*MAT_091 
*MAT_092 
*MAT_005 
*MAT_014 
*MAT_192 
*MAT_078 
*MAT_130 
*MAT_SPH_01 
*MAT_100 
*MAT_100_DA 
*MAT_211 
*MAT_S01 
*MAT_S03 
*MAT_S06 
*MAT_S08
ALPHABETIZED MATERIALS LIST  
Material Keyword 
Number 
*MAT_SPRING_MAXWELL 
*MAT_SPRING_MUSCLE 
*MAT_SPRING_NONLINEAR_ELASTIC 
*MAT_SPRING_SQUAT_SHEARWALL 
*MAT_SPRING_TRILINEAR_DEGRADING 
*MAT_STEEL_CONCENTRIC_BRACE 
*MAT_STEEL_EC3 
*MAT_STEINBERG 
*MAT_STEINBERG_LUND 
*MAT_STOUGHTON_NON_ASSOCIATED_FLOW 
*MAT_STRAIN_RATE_DEPENDENT_PLASTICITY 
*MAT_TABULATED_JOHNSON_COOK 
*MAT_S07 
*MAT_S15 
*MAT_S04 
*MAT_S14 
*MAT_S13 
*MAT_171 
*MAT_202 
*MAT_011 
*MAT_011_LUND 
*MAT_260A 
*MAT_019 
*MAT_224 
*MAT_TABULATED_JOHNSON_COOK_GYS 
*MAT_224_GYS 
*MAT_TABULATED_JOHNSON_COOK_ORTHO_PLASTICITY 
*MAT_264 
*MAT_TAILORED_PROPERTIES 
*MAT_TEMPERATURE_DEPENDENT_ORTHOTROPIC  
*MAT_THERMAL_CHEMICAL_REACTION 
*MAT_THERMAL_CWM 
*MAT_THERMAL_DISCRETE_BEAM 
*MAT_THERMAL_ISOTROPIC 
*MAT_THERMAL_ISOTROPIC_PHASE_CHANGE 
*MAT_THERMAL_ISOTROPIC_TD 
*MAT_THERMAL_ISOTROPIC_TD_LC 
*MAT_THERMAL_OPTION 
*MAT_THERMAL_ORTHOTROPIC 
*MAT_THERMAL_ORTHOTROPIC_TD 
*MAT_THERMAL_ORTHOTROPIC_TD_LC 
*MAT_THERMAL_USER_DEFINED 
*MAT_THERMO_ELASTO_VISCOPLASTIC_CREEP  
*MAT_TISSUE_DISPERSED  
LS-DYNA R10.0 
*MAT_251 
*MAT_023 
*MAT_T06 
*MAT_T07 
*MAT_T05 
*MAT_TO1 
*MAT_T09 
*MAT_T03 
*MAT_T10 
*MAT_T00 
*MAT_T02 
*MAT_T04 
*MAT_T08 
*MAT_T11 
*MAT_188
ALPHABETIZED MATERIALS LIST 
Material Keyword 
*MAT_TOUGHENED_ADHESIVE_POLYMER 
Number 
*MAT_252 
*MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLASTIC 
*MAT_037 
*MAT_TRANSVERSELY_ISOTROPIC_CRUSHABLE_FOAM 
*MAT_TRIP 
*MAT_UHS_STEEL 
*MAT_UNIFIED_CREEP 
*MAT_UNIFIED_CREEP_ORTHO 
*MAT_USER_DEFINED_MATERIAL_MODELS 
*MAT_VACUUM 
*MAT_VISCOELASTIC 
*MAT_VISCOELASTIC_FABRIC 
*MAT_VISCOELASTIC_HILL_FOAM 
*MAT_VISCOELASTIC_LOOSE_FABRIC  
*MAT_VISCOELASTIC_THERMAL 
*MAT_VISCOPLASTIC_MIXED_HARDENING 
*MAT_VISCOUS_FOAM 
*MAT_142 
*MAT_113 
*MAT_244 
*MAT_115 
*MAT_115_O 
*MAT_041-050 
*MAT_140 
*MAT_006 
*MAT_134 
*MAT_178 
*MAT_234 
*MAT_175 
*MAT_225 
*MAT_062 
*MAT_WINFRITH_CONCRETE_REINFORCEMENT 
*MAT_084_REINF 
*MAT_WINFRITH_CONCRETE 
*MAT_WOOD_{OPTION} 
*MAT_WTM_STM 
*MAT_WTM_STM_PLC 
*MAT_084 
*MAT_143 
*MAT_135 
*MAT_135_PLC
*MAT_ADD_AIRBAG_POROSITY_LEAKAGE 
This  command  allows  users  to  model  porosity  leakage  through  non-fabric  material 
when  such  material  is  used  as  part  of  control  volume,  airbag.    It  applies  to  both 
*AIRBAG_HYBRID and *AIRBAG_WANG_NEFSKE. 
  Card 1 
1 
2 
3 
4 
5 
Variable 
MID 
FLC/X2 
FAC/X3 
ELA 
FVOPT 
Type 
I 
F 
F 
F 
F 
8 
6 
X0 
F 
7 
X1 
F 
Default 
none 
none 
1.0 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
MID 
Material ID for which the porosity leakage property applies 
FLC/X2 
If X0≠0 and  X0≠1 
X2  is  one  of  the  coefficients  of  the  porosity  in  the  equation  of
Anagonye  and  Wang  [1999].    (Defined  below  in  description  for
X0/X1) 
If X0=0  
GE.0.0: X2,  in  this  context  named  FLC,  is  an  optional  fabric
porous leakage flow coefficient. 
LT.0.0:  |FLC|  is  the  load  curve  ID of  the  curve  defining  FLC 
versus time. 
If X0=1 
GE.0.0: See X0=0 above. 
LT.0.0:  |FLC|  is  the  load  curve  ID  defining  FLC  versus  the
stretching ratio defined as 𝑟𝑠 = 𝐴/𝐴0.  See notes below.
FAC/X3 
If X0 ≠ 0 and  X0 ≠ 1 
X3  is  one  of  the  coefficients  of  the  porosity  in  the  equation  of
Anagonye  and  Wang  [1999].    (Defined  below  in  description  for
X0/X1) 
If X0 = 0 and FVOPT < 7 
GE.0.0: X3,  in  this  context  named  FAC,  is  an  optional  fabric
characteristic parameter.
LT.0.0:  |FAC| is the load curve ID of the curve defining FAC 
versus absolute pressure. 
If X0 = 1 and FVOPT < 7 
GE.0.0: See X0 = 0 and FVOPT < 7 above. 
LT.0.0:  |FAC|  is  the  load  curve  ID  defining  FAC  versus  the
pressure  ratio  defined  as  𝑟𝑝 = 𝑃air/𝑃bag.    See  remark  3 
of *MAT_FABRIC. 
If (X0 = 0 or X0 = 1) and (FVOPT = 7 or FVOPT = 8) 
GE.0.0: See X0 = 0 and FVOPT < 7 above. 
LT.0.0:  FAC  defines  leakage  volume  flux  rate  versus  absolute
pressure.    The  volume  flux  (per  area)  rate  (per  time)
has  the  unit  of  velocity  and  it  is  equivalent  to  relative
porous gas speed. 
[
𝑑(Volflux)
𝑑𝑡
] =
[volume]
[area]
[time]
=
[length]
[time]
= [velocity],
ELA 
Effective leakage area for blocked fabric, ELA. 
LT.0.0: |ELA|  is  the  load  curve  ID  of  the  curve  defining  ELA
versus time.  The default value of zero assumes that no
leakage occurs.  A value of .10 would assume that 10%
of the blocked fabric is leaking gas. 
FVOPT 
Fabric venting option. 
EQ.1: Wang-Nefske formulas for venting through an orifice are
used.  Blockage is not considered. 
EQ.2: Wang-Nefske formulas for venting through an orifice are
used.  Blockage of venting area due to contact is consid-
ered. 
EQ.3: Leakage  formulas  of  Graefe,  Krummheuer,  and  Siejak
[1990] are used.  Blockage is not considered. 
EQ.4: Leakage  formulas  of  Graefe,  Krummheuer,  and  Siejak
[1990] are used.  Blockage of venting area due to contact
is considered. 
EQ.5: Leakage formulas based on flow through a porous media 
are used.  Blockage is not considered. 
EQ.6: Leakage formulas based on flow through a porous media
are used.  Blockage of venting area due to contact is con-
sidered.
EQ.7: Leakage is based on gas volume outflow versus pressure
load  curve  [Lian,  2000].    Blockage  is  not  considered.
Absolute pressure is used in the porous-velocity-versus-
pressure load curve, given as FAC. 
EQ.8: Leakage is based on gas volume outflow versus pressure
load  curve  [Lian  2000].    Blockage  of  venting  or  porous
area  due  to  contact  is  considered.    Absolute  pressure  is
used  in  the  porous-velocity-versus-pressure  load  curve, 
given as FAC. 
X0, X1 
Coefficients of Anagonye and Wang [1999] porosity equation for
the leakage area: 
𝐴leak = 𝐴0(𝑋0 + 𝑋1𝑟𝑠 + 𝑋2𝑟𝑝 + 𝑋3𝑟𝑠𝑟𝑝)
*MAT_ADD_COHESIVE 
The  ADD_COHESIVE  option  offers  the  possibility  to  use  a  selection  of  3-dimensional 
material models in LS-DYNA in conjunction with cohesive elements. 
Usually the cohesive elements (ELFORM = 19 and 20 of *SECTION_SOLID) can only be 
used  with  a  small  subset  of  materials  (41-50,  138,  184,  185,  186,  240).    But  with  this 
additional keyword, a bigger amount of standard 3-d material models can be used, that 
would only be available for solid elements in general.  Currently the following material 
models are supported: 1, 3, 4, 6, 15, 24, 41-50, 81, 82, 89, 96, 98, 103, 104, 105, 106, 107, 
115, 120, 123, 124, 141, 168, 173, 187, 188, 193, 224, 225, 252, and 255. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
ROFLG 
INTFAIL 
THICK 
Type 
I 
F 
F 
F 
Default 
none 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
PID 
Part ID for which the cohesive property applies. 
ROFLG 
Flag for whether density is specified per unit area or volume. 
EQ.0.0:  Density specified per unit volume (default). 
EQ.1.0:  Density specified per unit area for controlling the mass
of cohesive elements with an initial volume of zero. 
INTFAIL 
The  number  of  integration  points  required  for  the  cohesive 
element to be deleted.  If it is zero, the element won’t be deleted
even if it satisfies the failure criterion.  The value of INTFAIL may
range from 1 to 4, with 1 the recommended value. 
THICK 
Thickness of the adhesive layer.  
EQ.0.0:  The actual thickness of the cohesive element is used. 
GT.0.0:  User specified thickness.
*MAT 
Cohesive elements possess 3 kinematic variables, namely two relative displacements 𝛿1, 
𝛿2  in  tangential  directions  and  one  relative  displacement  𝛿3  in  normal  direction.    In  a 
corresponding  constitutive  model,  they  are  used  to  compute  3  associated  traction 
stresses 𝑡1, 𝑡2, and 𝑡3, e.g.  in the elastic case (*MAT_COHESIVE_ELASTIC): 
𝑡1
⎤ =
⎡
𝑡2
⎥
⎢
𝑡3⎦
⎣
𝐸𝑇
⎡
⎢
⎣
𝐸𝑇
⎤
⎥
𝐸𝑁⎦
𝛿1
⎤
⎡
𝛿2
⎥
⎢
𝛿3⎦
⎣
On  the  other  hand,  hypoelastic  3-d  material  models  for  standard  solid  elements  are 
formulated with respect to 6 independent strain rates and 6 associated stress rates, e.g.  
for isotropic elasticity (*MAT_ELASTIC): 
𝜎̇𝑥𝑥
⎤
⎡
𝜎̇𝑦𝑦
⎥
⎢
⎥
⎢
𝜎̇𝑧𝑧
⎥
⎢
𝜎̇𝑥𝑦
⎥
⎢
⎥
⎢
𝜎̇𝑦𝑧
⎥
⎢
𝜎̇𝑧𝑥⎦
⎣
=
(1 + 𝜈)(1 − 2𝜈)
1 − 𝜈
⎡
⎢
⎢
⎢
⎢
⎢
⎣
1 − 𝜈
1 − 𝜈
1 − 2𝜈
1 − 2𝜈
⎤
⎥
⎥
⎥
⎥
⎥
1 − 2𝜈⎦
𝜀̇𝑥𝑥
⎤
⎡
𝜀̇𝑦𝑦
⎥
⎢
⎥
⎢
𝜀̇𝑧𝑧
⎥
⎢
𝜀̇𝑥𝑦
⎥
⎢
⎥
⎢
𝜀̇𝑦𝑧
⎥
⎢
𝜀̇𝑧𝑥⎦
⎣
To  be  able  to  use  such  3-dimensional  material  models  in  a  cohesive  element 
environment,  an  assumption  is  necessary  to  transform  3  relative  displacements  to  6 
strain rates.  Therefore it is assumed that no lateral expansion and no in-plane shearing 
is possible for the cohesive element: 
𝛿1
⎤
⎡
𝛿2
⎥
⎢
𝛿3⎦
⎣
      →       
𝜀̇𝑥𝑥
⎤
⎡
𝜀̇𝑦𝑦
⎥
⎢
⎥
⎢
𝜀̇𝑧𝑧
⎥
⎢
𝜀̇𝑥𝑦
⎥
⎢
⎥
⎢
𝜀̇𝑦𝑧
⎥
⎢
𝜀̇𝑧𝑥⎦
⎣
=
⎤
⎡
⎥
⎢
𝛿 ̇
⎥
⎢
3/(𝑡 + 𝛿3)
⎥
⎢
⎥
⎢
⎥
⎢
𝛿 ̇
2/(𝑡 + 𝛿3)
⎥
⎢
𝛿 ̇
1/(𝑡 + 𝛿3)⎦
⎣
where 𝑡 is the initial thickness of the adhesive layer, see parameter THICK.  These strain 
rates are then used in a 3-d constitutive model to obtain new Cauchy stresses, where 3 
components can finally be used for the cohesive element: 
𝜎𝑥𝑥
⎤
⎡
𝜎𝑦𝑦
⎥
⎢
𝜎𝑧𝑧
⎥
⎢
⎥
⎢
𝜎𝑥𝑦
⎥
⎢
𝜎𝑦𝑧
⎥
⎢
𝜎𝑧𝑥⎦
⎣
        →         
𝑡1
⎤ =
⎡
𝑡2
⎥
⎢
𝑡3⎦
⎣
𝜎𝑧𝑥
⎥⎤  
⎢⎡
𝜎𝑦𝑧
𝜎𝑧𝑧⎦
⎣
If this keyword is used in combination with a 3-dimensional material model, the output 
to D3PLOT or ELOUT is organized as in other material models for cohesive elements, 
see e.g.  *MAT_184.  Instead of the usual six stress components, three traction stresses
are written into those databases.  The in-plane shear traction along the 1-2 edge replaces 
the x-stress, the orthogonal in-plane shear traction replaces the y-stress, and the traction 
in the normal direction replaces the z-stress.
*MAT 
Many  of  the  constitutive  models  in  LS-DYNA  do  not  allow  failure  and  erosion.    The 
ADD_EROSION  option  provides  a  way  of  including  failure  in  these  models.    This 
option  can  also  be  applied  to  constitutive  models  that  already  include  other 
failure/erosion criterion. 
For  the  non-damage  options,  each  of  the  failure  criteria  defined  here  are  applied 
independently, and once a sufficient number of those criteria are satisfied according to 
NCS, the element is deleted from the calculation.  
In  addition  to  erosion,  the  “generalized  incremental  stress-state  dependent  damage 
model” (GISSMO) or alternative “damage initiation and evolution models” (DIEM) are 
available as described in the remarks.  See variable IDAM.  For DIEM, NCS has a special 
meaning, see description below for details. 
This  option  applies  to  nonlinear  element  formulations  including  the  2D  continuum 
elements,  3D  solid  elements,  2D  and  3D  SPH  particles,  3D  shell  elements,  and  thick 
shell  elements.  Beam  formulations  1  and  11  currently  support  the  erosion  but  not  the 
damage and evolution models. 
NOTE: that  all  *MAT_ADD_EROSION  commands  in  a 
model can be disabled by using *CONTROL_MAT. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
EXCL 
MXPRES  MNEPS 
EFFEPS 
VOLEPS 
NUMFIP 
NCS 
Type 
A8 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
0.0 
0.0 
0.0 
0.0 
1.0 
1.0/0.0 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MNPRES 
SIGP1 
SIGVM 
MXEPS 
EPSSH 
SIGTH 
IMPULSE 
FAILTM 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none
*MAT_ADD_EROSION 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IDAM 
DMGTYP 
LCSDG 
ECRIT 
DMGEXP 
DCRIT 
FADEXP 
LCREGD 
Type 
A8 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
1.0 
0.0 
1.0 
0.0 
Additional card for IDAM > 0. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SIZFLG 
REFSZ 
NAHSV 
LCSRS 
SHRF 
BIAXF 
Type 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Damage Initiation and Evolution Card Pairs.  For IDAM < 0 include | IDAM | pairs 
of Cards 5 and 6. 
5 
6 
7 
8 
  Card 5 
1 
Variable 
DITYP 
Type 
F 
2 
P1 
F 
3 
P2 
F 
4 
P3 
F 
Default 
0.0 
0.0 
0.0 
0.0
6 
7 
8 
*MAT_ADD_EROSION 
  Card 6 
1 
2 
Variable 
DETYP 
DCTYP 
Type 
F 
F 
3 
Q1 
F 
4 
Q2 
F 
Default 
0.0 
0.0 
0.0 
0.0 
Optional Card with additional failure criteria. 
  Card 7 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCFLD 
EPSTHIN 
ENGCRT  RADCRT 
Type 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
MID 
EXCL 
DESCRIPTION
Material  identification  for  which  this  erosion  definition  applies.
A  unique  number  or  label  not  exceeding  8  characters  must  be
specified. 
The exclusion number, which applies to the failure values defined
on  Cards  1,  2,  and  7.    When  any  of  the  failure  values  on  these 
cards  are  set  to  the  exclusion  number,  the  associated  failure
criterion  is  not  invoked.    Or  in  other  words,  only  the  failure
values not set to the exclusion number are invoked.  The default
value  of  EXCL  is  0.0,  which  eliminates  all  failure  criteria  from 
consideration that have their constants left blank or set to 0.0.   
As  an  example,  to  prevent  a  material  from  developing  tensile
pressure,  the  user  could  specify  an  unusual  value  for  the
exclusion  number,  e.g.,  1234,  set  MNPRES  to  0.0,  and  set  all  the 
remaining  failure  values  to  1234.    However,  use  of  an  exclusion
number  may  be  considered  nonessential  since  the  same  effect
could be achieved without use of the exclusion number by setting
MNPRES to a very small negative value.
MXPRES 
*MAT_ADD_EROSION 
DESCRIPTION
Maximum pressure at failure, 𝑃max. If the value is exactly zero, it 
is  automatically  excluded  to  maintain  compatibility  with  old
input files. 
MNEPS 
Minimum  principal  strain  at  failure,  𝜀min.  If  the  value  is  exactly 
zero,  it  is  automatically  excluded  to  maintain  compatibility  with
old input files. 
EFFEPS 
Maximum effective strain at failure: 
𝜀eff = ∑ √
𝑖𝑗
dev𝜀𝑖𝑗
𝜀𝑖𝑗
dev
. 
If  the  value  is  exactly  zero,  it  is  automatically  excluded  to
maintain  compatibility  with  old  input  files.    If  the  value  is
negative,  then  |EFFEPS|  is  the  effective  plastic  strain  to  failure.
In combination with cohesive elements, EFFEPS is the maximum
effective in-plane strain. 
VOLEPS 
Volumetric strain at failure, 
or 
𝜀vol = 𝜀11 + 𝜀22 + 𝜀33, 
ln(relative volume). 
VOLEPS  can  be  a  positive  or  negative  number  depending  on
whether the failure is  in tension or compression, respectively.  If
the value is exactly zero, it is automatically excluded to maintain
compatibility with old input files.
VARIABLE   
NUMFIP 
DESCRIPTION
Number  of  failed  integration  points  prior  to  element  deletion.
The default is unity.  See Remark 10. 
LT.0.0 (IDAM = 0): Only 
is 
for  shells. 
  |NUMFIP| 
the 
percentage of integration points which must 
exceed  the  failure  criterion  before  element 
fails.    If  NUMFIP < -100,  then  |NUMFIP|-
100 is the number of failed integration points 
prior to element deletion. 
LT.0.0 (IDAM≠ 0):  Only 
is 
for  shells. 
  |NUMFIP| 
the 
percentage  of  layers  which  must  fail  before 
element  fails.    For  shell  formulations  with  4 
integration points per layer, the layer is con-
sidered failed if any of the integration points 
in the layer fails. 
NCS 
This  meaning  of  this  input  depends  on  whether  the  damage
option DIEM is used or not.  
IDAM.GE.0: Number  of  failure  conditions  to  satisfy  before
failure  occurs.    For  example,  if  SIGP1  and  SIGVM
are  defined  and  if  NCS = 2,  both  failure  criteria 
must  be  met  before  element  deletion  can  occur. 
The default is set to unity. 
IDAM.LT.0:  Plastic  strain  increment  between  evaluation  of
damage  instability  and  evolution  criteria.    See  DI-
EM description, the default is zero. 
MNPRES 
Minimum pressure at failure, 𝑃min. 
SIGP1 
SIGVM 
MXEPS 
EPSSH 
SIGTH 
Principal stress at failure, 𝜎max. 
Equivalent stress at failure, 𝜎̅̅̅̅̅max. The equivalent  stress at failure 
is made a function of the effective strain rate by setting SIGVM to
the negative of the appropriate load curve ID. 
Maximum  principal  strain  at  failure,  𝜀max.  The  maximum 
principal strain at failure is made a function of the effective strain
rate  by  setting  MXEPS  to  the  negative  of  the  appropriate  load
curve ID. 
Tensorial shear strain at failure, 𝛾max/2.   
Threshold stress, 𝜎0.
*MAT_ADD_EROSION 
DESCRIPTION
IMPULSE 
Stress impulse for failure, 𝐾f. 
FAILTM 
Failure time.  When the problem time exceeds the failure time, the
material is removed. 
IDAM 
Flag for damage model. 
EQ.0: no damage model is used. 
EQ.1: GISSMO damage model. 
LT.0:  -IDAM  represents  the  number  of  damage  initiation  and
evolution model (DIEM) criteria to be applied 
DMGTYP 
For GISSMO damage type the following applies.  
DMGTYP is interpreted digit-wise as follows: 
DMGTYP = [𝑁𝑀] = 𝑀 + 10 × 𝑁 
M.EQ.0: Damage is accumulated, no coupling to flow stress, no 
failure. 
M.EQ.1: Damage  is  accumulated,  element  failure  occurs  for
𝐷 = 1.  Coupling of damage to flow stress depending
on parameters, see remarks below.  
N.EQ.0:  Equivalent plastic strain is the driving quantity for the
damage.  (To be more precise, it’s the history variable
that LS-PrePost blindly labels as “plastic strain”.  What
this  history  variable  actually  represents  depends  on
the material model.) 
N.GT.0:  The  Nth  additional  history  variable  is  the  driving
quantity  for  damage.    These  additional  history  varri-
ables are the same ones flagged by the *DATABASE_-
EXTENT_BINARY  keyword’s  NEIPS  and  NEIPH 
fields.    For  example,  for  solid  elements  with  *MAT_-
187  setting  𝑁 = 6  chooses  volumetric  plastic  strain  as 
the driving quantity for the GISSMO damage. 
For IDAM.LT.0 the following applies. 
EQ.0:  No action is taken 
EQ.1:  Damage  history  is  initiated  based  on  values  of  initial
plastic  strains  and  initial  strain  tensor,  this  is  to  be
used in multistage analyses
VARIABLE   
LCSDG 
DESCRIPTION
Load curve ID or Table ID.  Load curve defines equivalent plastic
strain  to  failure  vs.    triaxiality.    Table  defines  for  each  Lode
parameter  value  (between  -1  and  1)  a  load  curve  ID  giving  the 
equivalent  plastic  strain  to  failure  vs.    triaxiality  for  that  Lode 
parameter value. 
ECRIT 
Critical plastic strain (material instability), see below. 
LT.0.0:  |ECRIT|  is  either  a  load  curve  ID  defining  critical
equivalent plastic strain versus triaxiality or a table ID
defining  critical  equivalent  plastic  strain  as  a  function 
of triaxiality and Lode parameter (as in LCSDG). 
EQ.0.0: Fixed  value  DCRIT  defining  critical  damage  is  read
 
GT.0.0:  Fixed  value 
for  stress-state 
independent  critical 
equivalent plastic strain. 
DMGEXP 
Exponent for nonlinear damage accumulation, see remarks. 
DCRIT 
Damage  threshold  value  (critical  damage).  If  a  Load  curve  of 
critical  plastic  strain  or  fixed  value  is  given  by  ECRIT,  input  is
ignored. 
FADEXP 
Exponent for damage-related stress fadeout. 
LCREGD 
LT.0.0:  |FADEXP|  is  load  curve  ID  defining  element-size 
dependent fading exponent. 
GT.0.0: Constant fading exponent. 
Load  curve  ID  defining  element  size  dependent  regularization
factors  for  equivalent  plastic  strain  to  failure  in  the  GISSMO
damage  model.    This  feature  can  also  be  used  with  the  standard 
(non-GISSMO)  failure  criteria  of  Cards  1  (MXPRES,  MNEPS,
EFFEPS, VOLEPS), 2 (MNPRES, SIGP1, SIGVM, MXEPS, EPSSH,
IMPULSE) and 4 (LCFLD, EPSTHIN), i.e.  when IDAM = 0.
*MAT_ADD_EROSION 
DESCRIPTION
SIZFLG 
Flag for method of element size determination. 
EQ.0: (default)  Element  size  is  determined  in  undeformed
configuration  as  square  root  of  element  area  (shells),  or
cubic root of element volume (solids), respectively. 
EQ.1: Element size is updated every time step, and determined
as  mean  edge  length  (this  option  was  added  to  ensure 
comparability with *MAT_120, and is not recommended 
for general purpose). 
Reference element size, for which an additional output of damage
will be generated.  This is necessary to ensure the applicability of
resulting  damage  quantities  when  transferred  to  different  mesh
sizes. 
Number  of  history  variables  from  damage  model  which  should 
be  stored  in  standard  material  history  array  for  Postprocessing.
See remarks. 
Load curve ID defining failure strain scaling factor for LCSDG vs.
strain rate.  If the first strain rate value in the curve is negative, it
is  assumed  that  all  strain  rate  values  are  given  as  natural
logarithm of the strain rate. The curve should not extrapolate to zero 
or failure may occur at low strain. 
GT.0: scale ECRIT, too 
LT.0:  do not scale ECRIT. 
Reduction factor for regularization at triaxiality = 0 (shear) 
Reduction factor for regularization at triaxiality = 2/3 (biaxial) 
Damage initiation type 
EQ.0.0: Ductile based on stress triaxiality 
EQ.1.0: Shear 
EQ.2.0: MSFLD 
EQ.3.0: FLD 
REFSZ 
NAHSV 
LCSRS 
SHRF 
BIAXF 
DITYP 
EQ.4.0: Ductile based on normalized principal stress  
P1 
Damage initiation parameter 
DITYP.EQ.0.0: Load  curve/table  ID  representing  plastic  strain
VARIABLE   
DESCRIPTION
at onset of damage as function of stress triaxiali-
ty 𝜂 and optionally plastic strain rate. 
DITYP.EQ.1.0: Load  curve/table  ID  representing  plastic  strain
at  onset  of  damage  as  function  of  shear  influ-
ence 𝜃 and optionally plastic strain rate. 
DITYP.EQ.2.0: Load  curve/table  ID  representing  plastic  strain
at  onset  of  damage  as  function  of  ratio  of  prin-
cipal plastic strain rates 𝛼 and optionally plastic 
strain rate. 
DITYP.EQ.3.0: Load  curve/table  ID  representing  plastic  strain
at  onset  of  damage  as  function  of  ratio  of  prin-
cipal plastic strain rates 𝛼 and optionally plastic 
strain rate. 
DITYP.EQ.4.0: Load  curve/table  ID  representing  plastic  strain
at onset of damage as function of stress state pa-
rameter 𝛽 and optionally plastic strain rate. 
P2 
Damage initiation parameter 
DITYP.EQ.0.0: Not used 
DITYP.EQ.1.0: Pressure influence parameter 𝑘𝑠 
DITYP.EQ.2.0: Layer specification 
EQ.0:  Mid layer 
EQ.1:  Outer layer 
DITYP.EQ.3.0: Layer specification 
EQ.0:  Mid layer 
EQ.1:  Outer layer 
DITYP.EQ.4.0: Triaxiality influence parameter 𝑘𝑑 
P3 
Damage initiation parameter 
DITYP.EQ.0.0: Not used 
DITYP.EQ.1.0: Not used 
DITYP.EQ.2.0: Initiation formulation 
EQ.0: Direct 
EQ.1: Incremental 
DITYP.EQ.3.0: Initiation formulation 
EQ.0:  Direct
DESCRIPTION
EQ.1:  Incremental 
DITYP.EQ.4.0:  Not used 
*MAT_ADD_EROSION 
DETYP 
Damage evolution type 
EQ.0.0: Linear  softening,  evolution  of  damage  is  a  function  of
the plastic displacement after the initiation of damage.
EQ.1.0: Linear  softening,  evolution  of  damage  is  a  function  of
the fracture energy after the initiation of damage. 
DCTYP 
Damage composition option for multiple criteria 
EQ.-1.0:  Damage not coupled to stress 
EQ.0.0:  Maximum 
EQ.1.0:  Multiplicative 
Q1 
Damage evolution parameter 
DETYP.EQ.0.0:  Plastic  displacement  at  failure, 𝑢𝑓
value corresponds to a table ID for 𝑢𝑓
tion of triaxiality and damage. 
𝑝,  a  negative 
𝑝 as a func-
Q2 
LCFLD 
DETYP.EQ.1.0:  Fracture energy at failure, 𝐺𝑓 . 
Set  to  1.0  to  output  information  to  log  files  (messag  and  d3hsp) 
when an integration point fails. 
Load curve ID or Table ID.  Load curve defines the Forming Limit
Diagram, where minor engineering strains in percent are defined
as  abscissa  values  and  major  engineering  strains  in  percent  are 
defined  as  ordinate  values.    Table  defines  for  each  strain  rate  an
associated  FLD  curve.    The  forming  limit  diagram  is  shown  in
Figure M39-1.  In defining the curve, list pairs of minor and major 
strains starting with the left most point and ending with the right
most point.  This criterion is only available for shell elements. 
EPSTHIN 
Thinning strain at failure for thin and thick shells.  
GT.0.0: individual  thinning  for  each  integration  point  from  𝑧-
strain 
LT.0.0:  averaged  thinning  strain  from  element  thickness
change
VARIABLE   
DESCRIPTION
ENGCRT 
Critical energy for nonlocal failure criterion, see Item 9 below. 
RADCRT 
Critical radius for nonlocal failure criterion, see Item 9 below. 
In addition to failure time, supported criteria for failure are: 
1.  𝑃 ≥ 𝑃max,  where  P  is  the  pressure  (positive  in  compression),  and  𝑃max  is  the 
maximum pressure at failure. 
2. 
𝜀3 ≤ 𝜀min, where 𝜀3 is the minimum principal strain, and 𝜀min is the minimum 
principal strain at failure. 
3.  𝑃 ≤ 𝑃min,  where  P  is  the  pressure  (positive  in  compression),  and  𝑃min  is  the 
minimum pressure at failure. 
4.  𝜎1 ≥ 𝜎max, where 𝜎1 is the maximum principal stress, and 𝜎maxis the maximum 
principal stress at failure. 
5.  √3
′ 𝜎𝑖𝑗
2 𝜎𝑖𝑗
′ ≥ 𝜎̅̅̅̅̅max, where 𝜎𝑖𝑗
equivalent stress at failure. 
′  are the deviatoric stress components, and 𝜎̅̅̅̅̅max is the 
6. 
𝜀1 ≥ 𝜀max, where 𝜀1 is the maximum principal strain, and 𝜀max is the maximum 
principal strain at failure. 
7.  𝛾1 ≥ 𝛾max/2, where 𝛾1 is the maximum tensorial shear strain = (𝜀1 − 𝜀3)/2, and 
𝛾max is the engineering shear strain at failure. 
8.  The Tuler-Butcher criterion, 
∫ [max(0, 𝜎1
− 𝜎0)]2dt ≥ Kf, 
where  𝜎1  is  the  maximum  principal  stress,  𝜎0  is  a  specified  threshold  stress, 
𝜎1 ≥ 𝜎0 ≥ 0,  and  Kf  is  the  stress  impulse  for  failure.    Stress  values  below  the 
threshold value are too low to cause fracture even for very long duration load-
ings. 
9.  A nonlocal failure criterion which is mainly intended for windshield impact can 
be defined via ENGCRT, RADCRT, and one additional “main” failure criterion 
(only  SIGP1  is  available  at  the  moment).    All  three  parameters  should  be  de-
fined for one part, namely the windshield glass and the glass should be discre-
tized with shell elements.  The course of events of this nonlocal failure model is 
as  follows:  If  the  main  failure  criterion  SIGP1  is  fulfilled,  the  corresponding 
element is flagged as  center of impact, but  no element erosion takes place yet.
Then, the internal energy of shells inside a circle, defined by RADCRT, around 
the  center  of  impact  is  tested  against  the  product  of  the  given  critical  energy 
ENGCRT and the “area factor”.  The area factor is defined as, 
Area Factor =
total area of shell elements found inside the circle
2𝜋 × RADCRT2
The  reason  for  having  two  times  the  circle  area  in  the  denominator  is  that  we 
expect two layers of shell elements, as would typically be the case for laminated 
windshield glass..  If this energy criterion is exceeded, all elements of the part 
are now allowed to be eroded by the main failure criterion. 
10.  When IDAM = 0, there are 3 ways to specify how shell elements are eroded and 
removed from the calculation. 
a)  When NUMFIP > 0, elements erode when NUMFIP points fail.  
b)  When  -100 ≤  NUMFIP <  0,  elements  erode  when  |NUMFIP|  percent  of 
the integration points fail.   
c)  When  NUMFIP <  -100,  elements  erode  when  |NUMFIP|-100  integration 
points fail.   
For NUMFIP > 0 and -100 ≤ NUMFIP < 0, layers retain full strength until the 
element is eroded.  For NUMFIP < -100, the stress at an integration point im-
mediately drops to zero when failure is detected at that integration point. 
When IDAM ≠ 0, there are 2 ways to specify how shell elements are eroded and 
removed from the calculation.   
a)  When NUMFIP > 0, elements erode when NUMFIP points fail.  
b)  When NUMFIP < 0, elements erode when |NUMFIP| percent of the lay-
ers fail.   
A layer fails if any integration point within that layer fails.  When IDAM = 0, 
erosion is in terms of failed points, not layers.
plastic
failure
strain
compression
-2/3
-1/3
tension
1/3
2/3
triaxiality
h/σ
vm
Figure 2-1.  Typical failure curve for metal sheet, modeled with shell elements.
DAMAGE MODELS 
GISSMO: 
The  GISSMO  damage  model  is  a  phenomenological  formulation  that  allows  for  an 
incremental description of damage accumulation, including softening and failure.  It is 
intended  to  provide  a  maximum  in  variability  for  the  description  of  damage  for  a 
variety of metallic materials (e.g.  *MAT_024, *MAT_036, *MAT_103, …).  The input of 
parameters is based on tabulated data, allowing the user to directly convert test data to 
numerical input. 
The model is based on an incremental formulation of damage accumulation: 
Δ𝐷 =
DMGEXP×𝐷
𝜀𝑓
(1−
DMGEXP
)
Δ𝜀𝑝 
where, 
𝐷 
𝜀𝑓  
Damage  value    (0 ≤ 𝐷 ≤ 1).  For  numerical  reasons,  𝐷  is  initialized  to  a 
value of 1.E-20 for all damage types in the first time step 
Equivalent plastic strain to failure, determined from LCSDG as a function 
of the current triaxiality value 𝜂 (and Lode parameter 𝐿 as an option). 
A  typical  failure  curve  LCSDG  for  metal  sheet,  modelled  with  shell  ele-
ments is shown in Figure 2-1 Triaxiality should be monotonically increas-
ing in this curve.  A reasonable range for triaxiality is -2/3 to 2/3 if shell 
elements are used (plane stress).
For  3-dimensional  stress  states  (solid  elements),  the  possible  range  of  tri-
axiality goes from −∞ to +∞, but to get a good resolution in the internal 
load  curve  discretization  (depending  on  parameter  LCINT  of  *CON-
TROL_SOLUTION)  one  should  define  lower  limits,  e.g.    -1  to  1  if 
LCINT = 100 (default). 
Δ𝜀𝑝 
Equivalent plastic strain increment 
For constant values of failure strain, this damage rate can be integrated to get a relation 
of damage and actual equivalent plastic strain: 
DMGEXP
𝐷 = (
𝜀𝑝
𝜀𝑓
)
,
for  𝜀𝑓 = constant 
Triaxiality 𝜂 as a measure of the current stress state is defined as 
𝜂 =
𝜎𝐻
𝜎𝑀
,
with hydrostatic stress 𝜎𝐻 and equivalent von Mises stress 𝜎𝑀. 
Lode parameter 𝐿 as an additional measure of the current stress state is defined as 
𝐿 =
27
𝐽3
𝜎𝑀
3 ,
with third invariant of the stress deviator 𝐽3. 
For DMGTYP.EQ.0, damage is accumulated according to the description above, yet no 
softening  and  failure  is  taken  into  account.    Thus,  parameters  ECRIT,  DCRIT  and 
FADEXP will not have any influence.  This option can be used to calculate pre-damage 
in multi-stage deformations without influencing the simulation results. 
For DMGTYP.EQ.1, elements will be deleted if D ≥ 1.  
Depending  on  the  set  of  parameters  given  by  ECRIT  (or  DCRIT)  and  FADEXP,  a 
Lemaitre-type coupling of damage and stress (effective stress concept) can be used. 
Three principal ways of damage definition can be used: 
1. 
Input of a fixed value of critical plastic strain (ECRIT.GT.0.) 
As soon as the magnitude of plastic strain reaches this value, the current dam-
age parameter 𝐷 is stored as critical damage DCRIT and the damage coupling 
flag is set to unity, in order to facilitate an identification of critical elements in 
postprocessing.    From  this  point  on,  damage  is  coupled  to  the  stress  tensor 
using the following relation: 
𝜎 = 𝜎̃  
⎢⎡1 − (
⎣
𝐷 − DCRIT
1 − DCRIT
FADEXP
)
⎥⎤ 
⎦
This  leads  to  a  continuous  reduction  of  stress,  up  to  the  load-bearing  capacity 
completely vanishing as 𝐷 reaches unity.  The fading exponent FADEXP can be
defined  element  size  dependent,  to  allow  for  the  consideration  of  an  element-
size dependent amount of energy to be dissipated during element fade-out. 
2. 
Input of a load curve defining critical plastic strain vs.  triaxiality (ECRIT < 0.), 
pointing  to  load  curve  ID  |ECRIT|.    This  allows  for  a  definition  of  triaxiality-
dependent material instability, which takes account of that instability and local-
ization will occur depending on the actual load case.  This offers the possibility 
to use a transformed Forming Limit Diagram as an input for the expected onset 
of softening and localization.  Using this load curve, the instability measure 𝐹 is 
accumulated using the following relation, which is similar to the accumulation 
of damage 𝐷 except for the instability curve is used as an input: 
Δ𝐹 =
DMGEXP
𝜀𝑝,𝑙𝑜𝑐
(1−
DMGEXP
)
Δ𝜀𝑝 
with, 
𝐹 
Instability measure (0 ≤ 𝐹 ≤ 1).  
𝜀p,loc  Equivalent plastic strain to instability, determined from ECRIT 
Δ𝜀𝑝 
Equivalent plastic strain increment 
As soon as the instability measure 𝐹 reaches unity, the current value of damage 
𝐷 in the respective element is stored.  Damage will from this point on be cou-
pled to the flow stress using the relation described above 
3. 
If no input for ECRIT is made, parameter DCRIT will be considered.  
Coupling of Damage to the stress tensor starts if this value (damage threshold) is 
exceeded  (0 ≤  DCRIT ≤  1).    Coupling  of  damage  to  stress  is  done  using  the 
relation described above. 
This input allows for the use of extreme values also – for example, DCRIT = 1.0 
would  lead  to  no  coupling  at  all,  and  element  deletion  under  full  load  (brittle 
fracture). 
History Variables: 
History  variables  of  the  GISSMO  damage  model  are  written  to  the  post-processing 
database  only  if  NAHSV >  0. 
  As  well,  NEIPH  and  NEIPS  must  be  set  in 
*DATABASE_EXTENT_BINARY.    The  damage  history  variables  start  at  position  ND, 
which  is  displayed  in  d3hsp  file,  e.g.    “first  damage  history  variable = 6”  means  that 
ND = 6.  For example, if you wish to view the damage parameter (first GISSMO history 
variable)  for  a  *MAT_024  shell  element,  you  must  set  NEIPS = 6  and  NAHSV = 1.    In 
LS-PrePost, access the damage parameter as history variable #6.
*MAT_ADD_EROSION 
ND  Damage parameter 𝐷, (10−20 < 𝐷 ≤ 1 ) 
  ND+1  Damage threshold DCRIT 
  ND+2  Domain flag for damage coupling (0: no coupling, 1: coupling)  
  ND+3 
Triaxiality variable 𝜎𝐻/𝜎𝑀 
  ND+4 
Equivalent plastic strain 
  ND+5  Regularization factor for failure strain (determined from LCREGD) 
  ND+6 
Exponent for stress fading FADEXP 
  ND+7  Calculated element size 
  ND+8 
Instability measure F 
  ND+9   Resultant damage parameter 𝐷 for element size REFSZ 
  ND+10  Resultant damage threshold DCRIT for element size REFSZ 
  ND+11  Averaged triaxiality 
  ND+12 
Lode parameter value (only calculated if LCSDG refers to a table) 
  ND+13  Alternative damage value: 𝐷1/DMGEXP 
  ND+14  Averaged Lode parameter 
DAMAGE INITIATION AND EVOLUTION CRITERIA: 
As  an  alternative  to  GISSMO,  the  user  may  invoke  up  to  5  damage  initiation  and 
evolution  criteria.    For  the  sake  of  efficiency,  the  parameter  NCS  can  be  used  to  only 
check  these  criteria  in  quantified  increments  of  plastic  strain.    In  other  words,  the 
criteria  are  only  checked  when  the  effective  plastic  strain  goes  beyond  NCS,  2 × NCS, 
3 × NCS, etc.  For NCS = 0 the checks are performed in each step there is plastic flow, a 
reasonable  value  of  NCS  could  for  instance  be  NCS = 0.0001.    The  following  theory 
applies to the DIEM option. 
Assuming  that  𝑛  initiation/evolution  types  have  been  specified  in  the  input  deck 
(𝑛 = −IDAM)  there  is  defined  at  each  integration  point  a  damage  initiation  variable, 
𝜔𝐷
𝑖 , and an evolution history variable 𝐷𝑖, such that, 
and 
𝑖 ∈ [0, ∞) 
𝜔𝐷
𝐷𝑖 ∈ [0,1],
𝑖 = 1, … 𝑛.
These are initially set to zero and evolve with the deformation of the elements according 
to  rules  associated  with  the  specific  damage  initiation  and  evolution  type  chosen,  see 
below for details. 
These quantities can be post-processed as ordinary material history variables and their 
positions in the history variables array is given in d3hsp, search for the string Damage 
history listing.  The damage initiation variables do not influence the results but serve to 
indicate  the  onset  of  damage.    As  an  alternative,  the  keyword  *DEFINE_MATERIAL_
HISTORIES can be used to output the instability and damage, following 
*DEFINE_MATERIAL_HISTORIES Properties 
Label 
Attributes 
Description 
Instability 
Damage 
- 
- 
- 
- 
- 
- 
-  Maximum 
initiation 
variable, 
𝑖  
max𝑖=1,…,𝑛 𝜔𝐷
- 
Effective damage 𝐷, see below 
The  damage  evolution  variables  govern  the  damage  in  the  material  and  are  used  to 
form the global damage 𝐷 ∈ [0,1].  Each criterion is of either of DCTYP set to maximum 
(DCTYP = 0) or multiplicative (DCTYP = 1), or one could choose to not couple damage 
to  the  stress  by  setting  DCTYP = −1.    This  means  that  the  damage  value  is  calculated 
and stored, but it is not affecting the stress as for the other options, so if all DCTYP are 
set  to  −1  there  will  be  no  damage  or  failure.    Letting  𝐼max  denote  the  set  of  evolution 
types  with  DCTYP  set  to  maximum  and  𝐼mult  denote  the  set  of  evolution  types  with 
DCTYP set to multiplicative the global damage, 𝐷, is defined as 
where 
and, 
𝐷 = max(𝐷max, 𝐷mult), 
𝐷max = max𝑖∈𝐼max𝐷𝑖 
𝐷mult = 1 − ∏ (1 − 𝐷𝑖)
. 
𝑖∈𝐼mult
The damage variable relates the macroscopic (damaged) to microscopic (true) stress by 
𝜎 = (1 − 𝐷)𝜎̃ . 
Once  the  damage  has  reached  the  level  of 𝐷erode  (=0.99  by  default)  the  stress  is  set  to 
zero  and  the  integration  point  is  assumed  failed  and  not  processed  thereafter.    For 
NUMFIP > 0,  a  shell  element  is  eroded  and  removed  from  the  finite  element  model 
when  NUMFIP  integration  points  have  failed.    For  NUMFIP < 0,  a  shell  element  is
eroded  and  removed  from  the  finite  element  model  when  -NUMFIP  percent  of  the 
layers have failed. 
DAMAGE INITIATION, ωD 
For  each  evolution  type 𝑖,  𝜔𝐷
𝜔𝐷
algorithms for modelling damage initiation. 
𝑖   is  independent  from  the  evolution  of 𝜔𝐷
𝑖   governs  the  onset  of  damage.    For 𝑖 ≠ 𝑗  the  evolution of 
𝑗 .    The  following  list  enumerates  the 
In this subsection we suppress the superscripted 𝑖 indexing the evolution type. 
Ductility Based on Stress Triaxiality (DITYP.EQ.0): 
For the ductile initiation option a function 𝜀𝐷
onset of damage (P1).  This is a function of stress triaxiality defined as 
𝑝 = 𝜀𝐷
𝑝 (𝜂, 𝜀̇𝑝) represents the plastic strain at 
𝜂 = −𝑝/𝑞 
with p being the pressure and q the von Mises equivalent stress.  Optionally this can be 
defined as a table with the second dependency being on the effective plastic strain rate 
𝜀̇𝑝. The damage initiation history variable evolves according to 
Shear (DITYP.EQ.1): 
𝜀𝑝
𝜔𝐷 = ∫
𝑑𝜀𝑝
𝜀𝐷
. 
For  the  shear  initiation  option  a  function 𝜀𝐷
onset of damage (P1).  This is a function of a shear stress function defined as 
𝑝 (𝜃, 𝜀̇𝑝)  represents  the  plastic  strain  at 
𝑝 = 𝜀𝐷
𝜃 = (𝑞 + 𝑘𝑆𝑝)/𝜏 
with p being the pressure, q the von Mises equivalent stress and τ the maximum shear 
stress defined as a function of the principal stress values 
𝜏 = (𝜎major − 𝜎minor)/2. 
Introduced here is also the pressure influence parameter 𝑘𝑠 (P2).  Optionally this can be 
defined as a table with the second dependency being on the effective plastic strain rate 
𝜀̇𝑝. The damage initiation history variable evolves according to 
𝜀𝑝
𝜔𝐷 = ∫
𝑑𝜀𝑝
𝜀𝐷
.
*MAT 
𝑝 (𝛼, 𝜀̇𝑝) represents the plastic strain at 
For the MSFLD initiation option a function 𝜀𝐷
onset  of  damage  (P1).    This  is  a  function  of  the  ratio  of  principal  plastic  strain  rates 
defined as 
𝑝 = 𝜀𝐷
𝛼 =
𝜀̇minor
𝜀̇major
. 
The  MSFLD  criterion  is  only  relevant  for  shells  and  the  principal  strains  should  be 
interpreted as the in-plane principal strains.  For simplicity the plastic strain evolution 
in this formula is assumed to stem from an associated von Mises flow rule and whence 
𝛼 =
𝑠minor
𝑠major
with  𝑠  being  the  deviatoric  stress.    This  insures  that  the  calculation  of  𝛼,  is  in  a  sense, 
robust  at  the  expense  of  being  slightly  innacurate  for  materials  with  anisotropic  yield 
functions  and/or  non-associated  flow  rules.    Optionally  this  can  be  defined  as  a  table 
with the second dependency being on the effective plastic strain rate 𝜀̇𝑝.  For 𝜀̇𝑝 = 0 the 
𝑝  is set to a large number to prevent onset of damage for no plastic evolution.  
value of 𝜀𝐷
Furthermore, the plastic strain used in this failure criteria is a modified effective plastic 
strain that only evolves when the pressure is negative, i.e., the material is not affected in 
compression. 
This  modified  plastic  strain  can  be  monitored  as  the  second  history  variable  of  the 
initiation  history  variables  in  the  binary  output  database.    For  P3 = 0,  the  damage 
initiation history variable is calculated directly from the ratio of (modified) plastic strain 
and the critical plastic strain 
𝜔𝐷 = max𝑡≤𝑇
𝜀𝑝
𝑝 . 
𝜀𝐷
This should be interpreted as the maximum value up to this point in time.  If P3 = 1 the 
damage  initiation  history  variable  is  instead  incrementally  updated  from  the  ratio  of 
(modified) plastic strain and the critical plastic strain 
𝜀𝑝
𝜔𝐷 = ∫
𝑑𝜀𝑝
𝜀𝐷
. 
For  this  initiation  option  P2  is  used  to  determine  the  layer  in  the  shell  where  the 
criterion is evaluated, if P2 = 0 the criterion is evaluated in the mid-layer only whereas if 
P2 = 1  it  is  evaluated  in  the  outer  layers  only  (bottom  and  top).    This  can  be  used  to 
distinguish between a membrane instability typically used for FLD evaluations (P2 = 0), 
and  a  bending  instability  (P2 = 1).    As  soon  as  𝜔𝐷  reaches  1  in  any  of  the  integration 
points  of  interest,  all  integration  points  in  the  shell  goes  over  in  damage  mode,  i.e., 
subsequent damage is applied to the entire element.
*MAT_ADD_EROSION 
The FLD initiation criterion is identical to MSFLD with one subtle difference: the plastic 
strain  used  for  evaluating  the  criteria  is  not  accounting  for  the  sign  of  the  hydrostatic 
stress, but is identical to the effective plastic strain directly from the underlying material 
model.  In other words, it is not the modified plastic strain used in the MSFLD criterion, 
but apart from that it is an identical criterion. 
Ductile based on normalized principal stress (DITYP.EQ.4): 
For the ductile initiation option the plastic strain at the onset of damage (P1) is taken as 
a function of 𝛽 and 𝜀̇𝑝, that is 𝜀𝐷
𝑝 (𝛽, 𝜀̇𝑝), where 𝛽 is the normalized principal stress 
𝑝 = 𝜀𝐷
𝛽 = (𝑞 + 𝑘𝑑𝑝)/𝜎major 
where 𝑝 is the pressure, 𝑞 is the von Mises equivalent stress, 𝜎major is the major principal 
stress,  and  where  𝑘𝑑  is  the  pressure  influence  parameter  specified  in  the  P2  field.  
Optionally,  this  can  be  defined  as  a  table  with  the  second  dependency  being  on  the 
effective plastic strain rate 𝜀̇𝑝. The damage initiation history variable evolves according 
to 
𝜀𝑝
𝜔𝐷 = ∫
𝑑𝜀𝑝
𝜀𝐷
. 
DAMAGE EVOLUTION, 𝑫 
For  the  evolution  of  the  associated  damage  variable  D  we  introduce  the  plastic 
displacement 𝑢𝑃 which evolves according to  
𝜔𝐷 < 1
𝑢̇𝑝 = {
𝑙𝜀̇𝑝 𝜔𝐷 ≥ 1
with 𝑙 being a characteristic length of the element.  Fracture energy is related to plastic 
displacement as follows 
𝑢𝑓
𝐺𝑓 = ∫ 𝜎𝑦𝑑𝑢̇𝑝
where 𝜎𝑦 is the yield stress.  The following list enumerates the algorithms available for 
modelling damage. 
Linear (DETYP.EQ.0): 
With this option the damage variable evolves linearly with the plastic displacement
𝑢̇𝑝
𝑝 
𝑢𝑓
𝑝 being the plastic displacement at failure (Q1).  If Q1 is negative, then –Q1 refers 
𝑝(𝜂, 𝐷), and 
𝑝 as a function of triaxiality and damage, i.e., 𝑢𝑓
with 𝑢𝑓
to a table that defines 𝑢𝑓
importantly the damage evolution law is changed generalized to 
𝑝 = 𝑢𝑓
𝐷̇ =
𝐷̇ =
𝑢̇𝑝
∂𝑢𝑓
∂𝐷
Linear (DETYP.EQ.1): 
With this option the damage variable evolves linearly as follows 
𝐷̇ =
𝑢̇𝑝
𝑝 
𝑢𝑓
where 𝑢𝑓
𝑝 = 2𝐺𝑓 /𝜎𝑦0 𝑢𝑓
𝑝 and 𝜎𝑦0 is the yield stress when failure criterion is reached.
*MAT_ADD_FATIGUE 
The ADD_FATIGUE option defines the S-N fatigue property of a material model. 
  Card 1 
1 
2 
3 
Variable 
MID 
LCID 
LTYPE 
Type 
I 
I 
Default 
none 
-1 
I 
0 
4 
A 
F 
5 
B 
F 
F 
I 
0 
I 
0 
0.0 
0.0 
none 
6 
7 
8 
STHRES 
SNLIMT 
SNTYPE 
S-N Curve Segment Cards.  Include one card for each additional S-N curve segment. 
Between zero and seven of these cards may be included in the deck.  This input ends at 
the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
Variable 
Type 
Default 
4 
Ai 
F 
5 
Bi 
F 
6 
7 
8 
STHRESi 
F 
0.0 
0.0 
none 
  VARIABLE   
DESCRIPTION
MID 
LCID 
Material identification for which the fatigue property applies. 
S-N fatigue curve ID. 
GT.0:  S-N fatigue curve ID 
EQ.-1:  S-N fatigue curve uses equation 𝑁𝑆𝑏 = 𝑎 
EQ.-2:  S-N fatigue curve uses equation log(𝑆) = 𝑎 − 𝑏 log(𝑁) 
EQ.-3:  S-N fatigue curve uses equation 𝑆 = 𝑎 𝑁𝑏 
LTYPE 
Type of S-N curve. 
EQ.0: Semi-log interpolation (default) 
EQ.1: Log-Log interpolation 
EQ.2:  Linear-Linear interpolation
VARIABLE   
DESCRIPTION
A 
B 
STHRES 
SNLIMT 
Material parameter 𝑎 in S-N fatigue equation. 
Material parameter 𝑏 in S-N fatigue equation. 
Fatigue  threshold  stress  if  the  S-N  curve  is  defined  by  equation 
(LCID < 0). 
If LCID > 0 
SNLIMNT  determines  the  algorithm  used  when  stress  is  lower
than the lowest stress on S-N curve. 
EQ.0: use the life at the last point on S-N curve 
EQ.1: extrapolation from the last two points on S-N curve 
EQ.2: infinity. 
If LCID < 0 
SNLIMIT  determines  the  algorithm  used  when  stress  is  lower
than STHRES. 
EQ.0: use the life at STHRES 
EQ.1: Ignored.  only applicable for LCID > 0 
EQ.2: infinity. 
SNTYPE 
Stress type of S-N curve. 
EQ.0: stress range (default) 
EQ.1: stress amplitude. 
Ai 
Bi 
Material parameter 𝑎 in S-N fatigue equation for the i-th segment.
Material parameter 𝑏 in S-N fatigue equation for the i-th segment.
STHRESi 
Fatigue threshold stress for the i-th segment. 
Remarks: 
1.  S-N curves can be defined by *DEFINE_CURVE, or for LCID < 0 by 
when LCID = -1 or for LCID = -2 
log(𝑆) = 𝑎 − 𝑏 log(𝑁) 
𝑁𝑆𝑏 = 𝑎 
or for LCID = -3
𝑆 
STHRES2
STHRES1
𝑁𝑆𝑏2 = 𝑎2
𝑁𝑆𝑏1 = 𝑎1 
𝑁 
Figure 2-2.  S-N Curve having multiple slopes 
𝑆 = 𝑎 𝑁𝑏 
where 𝑁 is the number of cycles for fatigue failure and 𝑆 is the stress amplitude.  
Note  that  the  two  equations  can  be  converted  to  each  other,  with  some  minor 
algebraic manipulation on the constants 𝑎 and 𝑏. 
To define S-N curve with multiple slopes, the S-N curve can be split into multi-
ple  segments  and  each  segment  is  defined  by  a  set  of  parameters  Ai,  Bi  and 
STHRESi.  Up to 8 sets of the parameters (Ai, Bi and STHRESi) can be defined.  
The  lower  limit  of  the  i-th  segment  is  represented  by  the  threshold  stress 
STHRESi, as shown in Figure 2-2.  This only applies to the case where the S-N 
curve is defined by equations (LCID = -1 or LCID = -2) 
2.  This  model  is  applicable  to  frequency  domain  fatigue  analysis,  defined  by  the 
keywords:  *FREQUENCY_DOMAIN_RANDOM_VIBRATION_FATIGUE,  and 
*FREQUENCY_DOMAIN_SSD_FATIGUE  .
*MAT_ADD_GENERALIZED_DAMAGE 
This option provides a way of including generalized (tensor type) damage and failure 
in  standard  LS-DYNA  material  models.    The  basic  idea  is  to  apply  a  general  damage 
model  (e.g.    GISSMO)  using  several  history  variables  as  damage  driving  quantities  at 
the same time.  With that feature it may be possible to obtain e.g.  anisotropic damage 
behavior or separate stress degradation for volumetric and deviatoric deformations.  A 
maximum  of  three  simultaneous  damage  evolutions  (i.e.    definition  of  3  history 
variables) is possible.  A detailed description of this model can be found in Erhart et al.  
[2017]. 
This  option  currently  applies  to  shell  element  types  1,  2,  3,  4,  16,  and  17  and  solid 
element types -2, -1, 1, 2, 3, 4, 10, 13, 15, 16, and 17. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
IDAM 
DTYP 
REFSZ 
NUMFIP 
PDDT 
NHIS 
Type 
I 
Default 
none 
  Card 2 
1 
I 
0 
2 
I 
0 
3 
F 
F 
0.0 
1.0 
4 
5 
6 
I 
0 
7 
I 
1 
8 
Variable 
HIS1 
HIS2 
HIS3 
IFLG1 
IFLG2 
IFLG3 
Type 
Default 
I 
0 
I 
I 
none 
none 
  Card 3 
1 
2 
3 
I 
0 
4 
I 
0 
5 
I 
0 
6 
Variable 
D11 
D22 
D33 
D44 
D55 
D66 
Type 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
7
(shells) 
*MAT_ADD_GENERALIZED_DAMAGE 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
D12 
D21 
D24 
D42 
D14 
D41 
Type 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
  Card 4 
   (solids) 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
D12 
D21 
D23 
D32 
D13 
D31 
Type 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
Damage definition cards for IDAM = 1 (GISSMO).  
2 x NHIS cards have to be defined, i.e.  two cards for each history variable. 
First Card for history variable HISn:  
Card 5… 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCSDG 
ECRIT 
DMGEXP 
DCRIT 
FADEXP 
LCREG 
Type 
Default 
I 
0 
F 
F 
F 
F 
0.0 
1.0 
0.0 
1.0 
I
Second Card for history variable HISn:  
Card 6… 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCSRS 
SHRF 
BIAXF 
LCDLIM 
Type 
Default 
I 
0 
F 
F 
0.0 
0.0 
I 
0 
  VARIABLE   
DESCRIPTION
MID 
Material ID for which this generalized damage definition applies.
IDAM 
Flag for damage model. 
EQ.0: no damage model is used. 
EQ.1: GISSMO damage model. 
DTYP 
Flag for damage behavior. 
EQ.0: Damage  is  accumulated,  no  coupling  to  flow  stress,  no
failure. 
EQ.1: Damage is accumulated, element failure occurs for D = 1.
REFSZ 
Reference element size, for which an additional output of damage
will be generated.  This is necessary to ensure the applicability of
resulting  damage  quantities  when  transferred  to  different  mesh
sizes. 
NUMFIP 
Number of failed integration points prior to element deletion.  
The default is unity. 
LT.0: |NUMFIP|  is  the  percentage  of  layers  which  must  fail
before element fails.
PDDT 
NHIS 
HISn 
*MAT_ADD_GENERALIZED_DAMAGE 
DESCRIPTION
Pre-defined  damage  tensors. 
  If  non-zero,  damage  tensor 
coefficients  D11  to  D66  on  cards  3  and  4  will  be  ignored.  See 
remarks for details. 
EQ.0:  No pre-defined damage tensor is used. 
EQ.1: 
Isotropic damage tensor. 
EQ.2:  2-parameter  isotropic  damage  tensor  for  volumetric-
deviatoric split. 
EQ.3:  Anisotropic  damage  tensor  as  in  MAT_104  (FLAG = -
1).  
EQ.4:  3-parameter damage tensor associated with IFLG1 = 2.
Number  of  history  variables  as  driving  quantities  (min = 1, 
max = 3).  
Choice of variable as driving quantity for damage, called “history
value” in the following.  
EQ.0:  Equivalent plastic strain rate is the driving quantity for
the  damage  if  IFLG1 = 0.    Alternatively  if  IFLG1 = 1, 
components of the plastic strain rate tensor are driving 
quantities for damage . 
GT.0:  The  rate  of  the  additional  history  variable  HISn  is  the
driving quantity for damage.  IFLG1 should be set to 0. 
LT.0: 
the  damage 
*DEFINE_FUNCTION 
driving  quantities  as  a  function  of  the  components  of 
the plastic strain rate tensor, IFLG1 should be set to 1. 
IDs  defining 
IFLG1 
Damage driving quantities  
EQ.0:  Rates of history variables HISn. 
EQ.1:  Specific components of the plastic strain rate tensor, see
remarks for details. 
EQ.2:  Predefined  functions  of  plastic  strain  rate  components 
for orthotropic damage model, HISn inputs will be ig-
nored, IFLG2 should be set to 1. This option is for shell 
elements only.
VARIABLE   
DESCRIPTION
IFLG2 
Damage strain coordinate system  
EQ.0:  Local element system (shells) or global system (solids).
EQ.1:  Material  system,  only  applicable  for  non-isotropic 
material models. Supported models for shells: all mate-
rials with AOPT feature.  Supported models for solids:
22, 33, 41-50, 103, 122, 157, 233. 
EQ.2:  Principal strain system (rotating). 
EQ.3:  Principal 
strain 
system 
(fixed  when 
instabil-
ity/coupling starts). 
IFLG3 
Erosion criteria and damage coupling system  
EQ.0:  Erosion  occurs  when  one  of  the  damage  parameters 
computed  reaches  unity,  the  damage  tensor  compo-
nents  are  based  on  the  individual  damage  parameters
d1 to d3. 
EQ.1:  Erosion  occurs  when  a  single  damage  parameter  D
reaches  unity,  the  damage  tensor  components  are
based on this single damage parameter. 
D11…D31 
LCSDG 
DEFINE_FUNCTION  IDs  for  damage  tensor  coefficients,  see
remarks. 
Load curve ID defining corresponding history value to failure vs.
triaxiality. 
ECRIT 
Critical history value (material instability), see below. 
LT.0.0:  |ECRIT|  is  load  curve  ID  defining  critical  history
value vs.  triaxiality. 
EQ.0.0: Fixed value DCRIT defining critical damage is read. 
GT.0.0:  Fixed value for stress-state independent critical history 
value. 
DMGEXP 
Exponent for nonlinear damage accumulation. 
DCRIT 
Damage  threshold  value  (critical  damage).  If  a  Load  curve  of 
critical  history  value  or  fixed  value  is  given  by  ECRIT,  input  is 
ignored.
*MAT_ADD_GENERALIZED_DAMAGE 
DESCRIPTION
FADEXP 
Exponent for damage-related stress fadeout. 
LT.0.0:  |FADEXP|  is  load  curve  ID  defining  element-size 
dependent fading exponent. 
GT.0.0: Constant fading exponent. 
LCREG 
LCSRS 
Load  curve  ID  defining  element  size  dependent  regularization
factors for history value to failure. 
Load  curve  ID  defining  failure  history  value  scaling  factor  for
LCSDG vs.  history value rate.  If the first rate value in the curve
is negative, it is assumed that all rate values are given as natural
logarithm of the history rate. 
GT.0: scale ECRIT, too 
LT.0:  do not scale ECRIT. 
SHRF 
Reduction factors for regularization at triaxiality = 0 (shear) 
BIAXF 
Reduction factors for regularization at triaxiality = 2/3 (biaxial) 
Load  curve  ID  defining  damage  limit  values  as  a  function  of
triaxiality.    Damage  can  be  restricted  to  values  less  than  1.0  to
for  certain
prevent 
triaxialities. 
further  stress  reduction  and 
failure 
LCDLIM 
Remarks: 
The GISSMO damage model is described in detail in the remarks of *MAT_ADD_ERO-
SION.  If NHIS = 1 and HIS1 = 0 is used, this new feature (“MAGD”) behaves  just the 
same as before (“GISSMO”).  The main difference with this new keyword is that up to 3 
independent but simultaneous damage evolutions are possible.  Therefore, parameters 
LCSDG,  ECRIT,  DMGEXP,  DCRIT,  FADEXP,  LCREGD,  LCSRS,  SHRF,  BIAXF,  and 
LCDLIM can be defined separately for each history variable. 
The  relation  between  nominal  (damaged)  stresses  𝜎𝑖𝑗  and  effective  (undamaged) 
stresses 𝜎̃𝑖𝑗 is now expressed as 
𝜎11
⎤
⎡
𝜎22
⎥
⎢
𝜎33
⎥
⎢
⎥
⎢
𝜎12
⎥
⎢
⎥
⎢
𝜎23
𝜎31⎦
⎣
=
𝐷11 𝐷12 𝐷13
⎡
𝐷21 𝐷22 𝐷23
⎢
⎢
𝐷31 𝐷32 𝐷33
⎢
⎢
⎢
⎢
⎣
0 𝐷44
𝐷55
⎤
⎥
⎥
⎥
⎥
⎥
⎥
𝐷66⎦
𝜎̃11
⎤
⎡
𝜎̃22
⎥
⎢
⎥
⎢
𝜎̃33
⎥
⎢
⎥
⎢
𝜎̃12
⎥
⎢
𝜎̃23
⎥
⎢
𝜎̃31⎦
⎣
with  damage  tensor  𝐷.    Each  damage  tensor  coefficient  𝐷𝑖𝑗  can  be  defined  via  *DE-
FINE_FUNCTION  as  a  function  of  damage  parameters  𝑑1  to  𝑑3.    For  simple  isotropic 
damage  driven  by  plastic  strain  (NHIS = 1,  HIS1 = 0,  IFLG1 = IFLG2 = IFLG3 = 0)  that 
would be 
𝜎11
⎤
⎡
𝜎22
⎥
⎢
𝜎33
⎥
⎢
⎥
⎢
𝜎12
⎥
⎢
⎥
⎢
𝜎23
𝜎31⎦
⎣
= (1 − 𝑑1)
⎡
⎢
⎢
⎢
⎢
⎢
⎣
⎤
⎥
⎥
⎥
⎥
⎥
1⎦
𝜎̃11
⎤
⎡
𝜎̃22
⎥
⎢
⎥
⎢
𝜎̃33
⎥
⎢
⎥
⎢
𝜎̃12
⎥
⎢
𝜎̃23
⎥
⎢
𝜎̃31⎦
⎣
That means the following function should be defined for D11 to D66 (Card 3): 
*DEFINE_FUNCTION 
1,D11toD66 
func1(d1,d2,d3)=(1.0-d1)  
and all entries in Card 4 can be left empty or equal zero in that case. 
If  GISSMO  (IDAM = 1)  is  used,  the  damage  parameters  used  in  those  functions  are 
internally replaced by 
𝑑𝑖      →        (
𝑑𝑖 − 𝐷𝐶𝑅𝐼𝑇𝑖
1 − 𝐷𝐶𝑅𝐼𝑇𝑖
𝐹𝐴𝐷𝐸𝑋𝑃𝑖
)
In the case of plane stress (shell) elements, coupling between normal stresses and shear 
stresses is implemented and the damage tensor is defined as below : 
𝜎11
⎤
⎡
𝜎22
⎥
⎢
⎥
⎢
⎥
⎢
𝜎12
⎥
⎢
⎥
⎢
𝜎23
𝜎31⎦
⎣
=
𝐷11 𝐷12
⎡
𝐷21 𝐷22
⎢
⎢
⎢
⎢
𝐷41 𝐷42
⎢
⎢
⎣
0 𝐷14
0 𝐷24
𝐷33
0 𝐷44
𝐷55
⎤
⎥
⎥
⎥
⎥
⎥
⎥
𝐷66⎦
𝜎̃11
⎤
⎡
𝜎̃22
⎥
⎢
⎥
⎢
⎥
⎢
𝜎̃12
⎥
⎢
𝜎̃23
⎥
⎢
𝜎̃31⎦
⎣
Since the evaluation of *DEFINE_FUNCTION for variables D11 to D66 is relatively time 
consuming, pre-defined damage tensors (PDDT) can be used.  Currently the following 
options are available for shell elements: 
PDDT = 1 
(1 − 𝐷1)
⎡
⎢
⎢
⎢
⎢
⎢
⎣
⎤
⎥
⎥
⎥
⎥
⎥
1⎦
PDDT = 3 
PDDT = 4 
*MAT_ADD_GENERALIZED_DAMAGE 
𝐷1 − 1
𝐷2
𝐷2
⎡1 − 2
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
𝐷1 − 1
𝐷2
𝐷1 − 1
1 − 2
𝐷2
𝐷1 − 1
1 − 𝐷1
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
1⎦
1 − 𝐷1
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
1 − 𝐷2
1 − 1
(𝐷1 + 𝐷2)
1 − 1
𝐷2
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
1 − 1
𝐷1⎦
1 − 𝐷1
⎡
⎢
⎢
⎢
⎢
⎢
⎣
1 − 𝐷2
1 − 𝐷3
⎤
⎥
⎥
⎥
⎥
⎥
1⎦
and the following ones for solid elements: 
PDDT = 
1 
PDDT = 
2 
𝐷1 − 1
𝐷2
𝐷2
𝐷2
⎡1 − 2
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
𝐷1 − 1
𝐷1 − 1
(1 − 𝐷1)
⎡
⎢
⎢
⎢
⎢
⎢
⎣
⎤
⎥
⎥
⎥
⎥
⎥
1⎦
𝐷1 − 1
1 − 2
𝐷2
𝐷1 − 1
𝐷2
𝐷2
𝐷1 − 1
1 − 2
𝐷1 − 1
𝐷1 − 1
𝐷2
𝐷2
𝐷1 − 1
𝐷2
1 − 𝐷1
1 − 𝐷1
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
1 − 𝐷1⎦
3 
1 − 𝐷1
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
1 − 𝐷2
1 − 𝐷3
1 − 1
(𝐷1 + 𝐷2)
*MAT 
⎤
1 − 1
(𝐷2 + 𝐷3)
1 − 1
(𝐷3 + 𝐷1)⎦
History Variables: 
The  increment  of  the  damage  parameter  is  computed  in  GISSMO  based  on  a  driving 
quantity that has the dimension of a strain rate : 
˙
𝑑˙ = 𝑛𝑑1−1 𝑛⁄ 𝐻𝐼𝑆𝚤
𝑒𝑝𝑓
The history variables defined by the user through HISi should thus have the dimension 
of  a  strain  as  the  rate  is  computed  internally  by  MAT_ADD_GENERALIZED_DAM-
AGE: 
HISı̇ =
HISi(𝑡𝑛+1) − HISi(𝑡𝑛)
𝑡𝑛+1 − 𝑡𝑛
History  variables  can  either  come  directly  from  associated  material  models  (IFLG1 = 0 
and  HISi > 0),  or  they  can  be  equivalent  to  plastic  strain  rate  tensor  components 
(IFLG1 = 1 and HISi = 0):  
HIṠ 1 = 𝜀̇𝑥𝑥
𝑝 , HIṠ 2 = 𝜀̇𝑥𝑥
𝑝 , HIṠ 3 = 𝜀̇𝑥𝑦
𝑝             (IFLG2 = 0) 
HIṠ 1 = 𝜀̇𝑎𝑎
𝑝 , HIṠ 2 = 𝜀̇𝑏𝑏
𝑝, HIṠ 2 = 𝜀̇2
𝑝             (IFLG2 = 1) 
𝑝 , HIṠ 3 = 𝜀̇𝑎𝑏
𝑝, HIṠ 3 = 0           (IFLG2 = 2) 
HIṠ 1 = 𝜀̇1
or  they  can  be  provided  via  *DEFINE_FUNCTIONs  by  the  user  (IFLG1 = 1  and 
HISi < 0): 
HIṠ
𝑖 = 𝑓𝑖(𝜀̇𝑥𝑥
𝑝 , 𝜀̇𝑦𝑦
𝑝 , 𝜀̇𝑧𝑧
𝑝 , 𝜀̇𝑥𝑦
𝑝 , 𝜀̇𝑦𝑧
𝑝 , 𝜀̇𝑧𝑥
𝑝 )            (IFLG2 = 0) 
HIṠ
𝑖 = 𝑓𝑖(𝜀̇𝑎𝑎
𝑝 , 𝜀̇𝑏𝑏
𝑝 , 𝜀̇𝑧𝑧
𝑝 , 𝜀̇𝑎𝑏
𝑝 , 𝜀̇𝑏𝑧
𝑝 , 𝜀̇𝑧𝑎
𝑝 )            (IFLG2 = 1) 
HIṠ
𝑖 = 𝑓𝑖(𝜀̇1
𝑝, 𝜀̇2
𝑝)           (IFLG2 = 2) 
e.g.    the  following  example  defines  a  history  variable  (HISi = -1234)  as  function  of  the 
transverse shear strains in material coordinate system a-b-z for shells:
*DEFINE_FUNCTION 
      1234 
fhis1(eaa,ebb,ezz,eab,ebz,eza)=1.1547*sqrt(ebz**2+eza**2)  
The plastic strain rate tensor is not always available in the material law and is estimated 
as: 
𝛆̇𝑝 =
𝜀̇𝑒𝑓𝑓
𝜀̇𝑒𝑓𝑓
[𝛆̇ −
𝜀̇𝒗𝒐𝒍
𝛅] 
This  is  a  good  approximation  for  isochoric  materials  with  small  elastic  strains  (e.g.  
metals) and correct for J2 plasticity. 
The following table gives an overview of the driving quantities used for incrementing 
the  damage  in  function  of  the  input  parameters  (strain  superscript  “p”  for  “plastic”  is 
omitted for convenience): 
IFLG1 
IFLG2 
HISi  >  0 
HISi  =  0 
HISi  <  0 
0 
0 
0 
1 
1 
1 
2 
2 
2 
0 
1 
2 
0 
1 
2 
0 
1 
2 
˙
HISı
˙
HISı
˙
HISı
N/A 
N/A 
N/A 
𝜀˙
N/A 
N/A 
𝜀˙𝑖𝑗
𝑚𝑎𝑡 
𝜀˙𝑖𝑗
𝜀˙𝑖
N/A 
N/A 
N/A 
𝑓 (𝜀˙𝑖𝑗) 
𝑓 (𝜀˙𝑖𝑗
𝑚𝑎𝑡) 
𝑓 (𝜀˙𝑖) 
N/A 
Preprogrammed  functions of plastic strain rate 
N/A 
Postprocessing History Variables: 
History  variables  of  the  GENERALIZED_DAMAGE  model  are  written  to  the  post-
processing database behind those already occupied by the material model which is used 
in combination:  
  Variable  Description 
ND 
Triaxiality variable 𝜎𝐻/𝜎𝑀 
  ND+1 
Lode parameter value 
  ND+2 
Single damage parameter 𝐷, (10−20 < 𝐷 ≤ 1 ), only for IFLG3 = 1
ND+3  Damage parameter 𝑑1 
  ND+4  Damage parameter 𝑑2 
  ND+5  Damage parameter 𝑑3 
  ND+6  Damage threshold DCRIT1 
  ND+7  Damage threshold DCRIT2 
  ND+8  Damage threshold DCRIT3 
  ND+12  History variable HIS1 
  ND+13  History variable HIS2 
  ND+14  History variable HIS3 
  ND+15  Angle between principal and material axes 
  ND+21  Characteristic element size (used in LCREG)  
For  instance,  ND = 6  for  *MAT_024,  ND = 9  for  *MAT_036,  or  ND = 23  for  *MAT_187.  
Exact information of the variable locations can be  found in the d3hsp  section “MAGD 
damage history listing”.
For consolidation calculations. 
*MAT_ADD_PERMEABILITY 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
PERM 
(blank) 
(blank) 
THEXP 
LCKZ 
Type 
I 
F 
F 
I 
Default 
none 
none 
0.0 
none 
  VARIABLE   
DESCRIPTION
MID 
Material identification – must be same as the structural material. 
PERM 
Permeability 
THEXP 
Undrained volumetric thermal expansion coefficient  
(Units:  1/temperature).    If  negative,  then  –THEXP  is  the  ID  of  a 
loadcurve  giving  thermal  expansion  coefficient  (y-axis)  versus 
temperature (x-axis). 
LCKZ 
Loadcurve giving factor on PERM versus z-coordinate.   
(X-axis – z-coordinate, yaxis – non dimensional factor) 
Remarks: 
The  units  of  PERM  are  length/time  (volume  flow  rate  of  water  per  unit  area  per 
gradient of pore pressure head). 
THEXP  represents  the  thermal  expansion  of  the  material  caused  by  the  pore  fluid.    It 
should be set equal to nαw, where n is the porosity of the soil and αw is the volumetric 
thermal  expansion  coefficient  of  the  pore  fluid.    If  the  pore  fluid  is  water,  the  thermal 
expansion  coefficient  varies  strongly  with  temperature;  a  curve  of  coefficient  versus 
temperature may be input instead of a constant value. 
See notes under *CONTROL_PORE_FLUID
For pore air pressure calculations. 
*MAT 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
PA_RHO 
PA_PRE 
PORE 
Type 
I 
I 
F 
F 
Default 
none  AIR_RO  AIR_RO
1. 
Remarks 
1 
1, 2 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PERM1 
PERM2 
PERM3 
CDARCY 
CDF 
LCPGD1 
LCPGD2 
LCPGD3 
Type 
F 
F 
F 
F 
F 
I 
I 
I 
Default 
0. 
PERM1  PERM1
1. 
0. 
none  LCPGD1 LCPGD1
Remarks  2, 3, 4, 5  2, 3, 4, 5  2, 3, 4, 5
1 
1, 5 
6 
6 
6 
  VARIABLE   
DESCRIPTION
MID 
Material identification – must be same as the structural material. 
PA_RHO 
PA_PRE 
Initial  density  of  pore  air,  default  to  atmospheric  air  density,
AIR_RO, defined in *CONTROL_PORE_AIR 
Initial  pressure  of  pore  air,  default  to  atmospheric  air  pressure,
AIR_P, defined in *CONTROL_PORE_AIR 
PORE 
Porosity, ratio of pores to total volume, default to 1.  
PERM[1-3] 
Permeability of pore air along 𝑥, 𝑦 and 𝑧-direction.  If less than 0 –
PERM[1-3]  is  taken  to  be  the  curve  ID  defining  the  permeability
coefficient  as  a  function  of  volume  ratio  of  current  volume  to
volume in the stress free state.
*MAT_ADD_PORE_AIR 
DESCRIPTION
CDARCY 
Coefficient of Darcy’s law 
CDF 
Coefficient of Dupuit-Forchheimer law 
LCPGD1~3 
Curves  defining  non-linear  Darcy’s  laws  along  x,  y  and  z-
directions, see Remarks 6. 
Remarks: 
1.  Card 1.  This card must be defined for all materials requiring consideration of 
pore  air  pressure.    The  pressure  contribution  of  pore  air  is  (𝜌 − 𝜌atm)RT×
PORE, where 𝜌 and 𝜌atm are the current and atmospheric air density, 𝑅 is air’s 
gas constant, 𝑇 is atmospheric air temperature and PORE is the porosity.  The 
values for 𝑅, 𝑇 and PORE are assumed to be constant during simulation. 
2.  Permeability  Model.   The  unit  of  PERMi  is  [Length]3[time]/[mass],  (air  flow 
velocity per gradient of excess pore pressure), i.e. 
(CDARCY + CDF × |𝑣𝑖|) × PORE × 𝑣𝑖 = PERM𝑖 ×
𝜕𝑃𝑎
𝜕𝑥𝑖
,
𝑖 = 1,2,3 
where 𝑣i is the pore air flow velocity along the ith direction, 𝜕𝑃𝑎/𝜕𝑥𝑖 is the pore 
air pressure gradient along the ith direction, and 𝑥1 = 𝑥, 𝑥2 = 𝑦, 𝑥3 = 𝑧. 
3.  Default Values for PERM2 and PERM3.  PERM2 and PERM3 are assumed to 
be  equal  to  PERM1  when  they  are  not  defined.    A  definition  of  “0”  means  no 
permeability. 
4.  Local  Coordinate  Systems.    (x,y,z),  or  (1,2,3),  refers  to  the  local  material 
coordinate system (a,b,c) when MID is an orthotropic material, such as *MAT_-
002 or *MAT_142; otherwise it refers to the global coordinate system. 
5.  CDF  for  Viscosity.    CDF  can  be  used  to  consider  the  viscosity  effect  for  high 
speed air flow 
6.  Nonlinearity.    LCPGDi  can  be  used  to  define  a  non-linear  Darcy’s  law  as 
follows: 
(CDARCY + CDF × |𝑣𝑖|) × PORE × 𝑣𝑖 = PERM𝑖 × 𝑓𝑖
𝜕𝑃𝑎
𝜕𝑥𝑖
,
𝑖 = 1,2,3 
where 𝑓𝑖 is value of the function defined  by the LCPGDi field.   The linear ver-
siono Darcy’s law of Remark 2, can be recovered when the LCPGDi curves are 
defined as straight lines of slope of 1.
*MAT 
The  ADD_THERMAL_EXPANSION  option  is  used  to  occupy  an  arbitrary  material 
model  in  LS-DYNA  with  a  thermal  expansion  property.    This  option  applies  to  all 
nonlinear  solid,  shell,  thick  shell  and  beam  elements  and  all  material  models  except 
those models which use resultant formulations such as *MAT_RESULTANT_PLASTIC-
ITY  and 
  Orthotropic  expansion  effects  are 
supported for anisotropic materials. 
  *MAT_SPECIAL_ORTHOTROPIC. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
LCID 
MULT 
LCIDY 
MULTY 
LCIDZ 
MULTZ 
Type 
I 
I 
F 
I 
F 
I 
F 
Default 
none 
none 
1.0 
LCID  MULT 
LCID  MULT 
  VARIABLE   
DESCRIPTION
PID 
LCID 
MULT 
LCIDY 
Part ID for which the thermal expansion property applies 
For  isotropic  material  models,  LCIDY,  MULTY,  LCIDZ,  and
MULTZ are ignored, and LCID is the load curve ID defining the
thermal  expansion  coefficient  as  a  function  of  temperature.    If
zero,  the  thermal  expansion  coefficient  is  constant  and  equal  to
MULT.  For anisotropic material models, LCID and MULT define
the thermal expansion coefficient in the local material a-direction.  
Scale factor scaling load curve given by LCID. 
Load curve ID defining the thermal expansion coefficient in local
material  b-direction  as  a  function  of  temperature.    If  zero,  the
thermal  expansion  coefficient  in  the  local  material  b-direction  is 
constant and equal to MULTY.  If MULTY = 0 as well, LCID and 
MULT  define  the  thermal  expansion  coefficient  in  the  local
material b-direction. 
MULTY 
Scale factor scaling load curve given by LCIDY.
LCIDZ 
*MAT_ADD_THERMAL_EXPANSION 
DESCRIPTION
Load curve ID defining the thermal expansion coefficient in local
material  c-direction  as  a  function  of  temperature.    If  zero,  the
thermal  expansion  coefficient  in  the  local  material  c-direction  is 
constant and equal to MULTZ.  If MULTZ = 0 as well, LCID and 
MULT  define  the  thermal  expansion  coefficient  in  the  local
material c-direction. 
MULTZ 
Scale factor scaling load curve given by LCIDZ. 
Remarks: 
When  invoking  the  isotropic  thermal  expansion  property  (no  use  of  the  local  y  and  z 
parameters) for a material, the stress update is based on the elastic strain rates given by 
𝑒 = 𝜀̇𝑖𝑗 − 𝛼(𝑇)𝑇̇𝛿𝑖𝑗 
𝜀̇𝑖𝑗
rather  than  on  the  total  strain  rates  𝜀̇𝑖𝑗.  For  a  material  with  the  stress  based  on  the 
deformation  gradient  𝐹𝑖𝑗,  the  elastic  part  of  the  deformation  gradient  is  used  for  the 
stress computations 
𝑒 = 𝐽𝑇
𝐹𝑖𝑗
−1/3𝐹𝑖𝑗 
where 𝐽𝑇 is the thermal Jacobian.  The thermal Jacobian is updated using the rate given 
by  
𝐽 ̇𝑇 = 3𝛼(𝑇)𝑇̇𝐽𝑇. 
For  orthotropic  properties,  which  apply  only  to  materials  with  anisotropy,  these 
equations are generalized to 
and 
where the 𝛽𝑖 are updated as 
𝑒 = 𝜀̇𝑖𝑗 − 𝛼𝑘(𝑇)𝑇̇𝑞𝑖𝑘𝑞𝑗𝑘 
𝜀̇𝑖𝑗
𝑒 = 𝐹𝑖𝑘𝛽𝑙
𝐹𝑖𝑗
−1𝑄𝑘𝑙𝑄𝑗𝑙 
𝛽̇
𝑖 = 𝛼𝑖(𝑇)𝑇̇𝛽𝑖. 
Here  𝑞𝑖𝑗  represents  the  matrix  with  material  directions  with  respect  to  the  current 
configuration  whereas  𝑄𝑖𝑗  are  the  corresponding  directions  with  respect  to  the  initial 
configuration.    For  (shell)  materials  with  multiple  layers  of  different  anisotropy 
directions, the mid surface layer determines the orthotropy for the thermal expansion.
*MAT 
In  nonlocal  failure  theories,  the  failure  criterion  depends  on  the  state  of  the  material 
within  a  radius  of  influence  which  surrounds  the  integration  point.    An  advantage  of 
nonlocal  failure  is  that  mesh  size  sensitivity  on  failure  is  greatly  reduced  leading  to 
results which converge to a unique solution as the mesh is refined. 
Without  a  nonlocal  criterion,  strains  will  tend  to  localize  randomly  with  mesh 
refinement  leading  to results  which  can  change  significantly  from  mesh  to  mesh.    The 
nonlocal failure treatment can be a great help in predicting the onset and the evolution 
of  material  failure.    This  option  can  be  used  with  two  and  three-dimensional  solid 
elements,  and  three-dimensional  shell  elements  and  thick  shell  elements.    This  option 
applies  to  a  subset  of  elastoplastic  materials  that  include  a  damage-based  failure 
criterion. 
  Card 1 
1 
2 
Variable 
IDNL 
PID 
Type 
I 
I 
3 
P 
F 
4 
Q 
F 
5 
L 
F 
6 
7 
8 
NFREQ 
NHV 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
History Cards.  Include as many cards as needed to set NHV variables. One card 2 will 
be read even if NHV = 0. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NL1 
NL2 
NL3 
NL4 
NL5 
NL6 
NL7 
NL8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none
Symmetry  Plane  Cards.    Define  one  card  for  each  symmetry  plane.    Up  to  six 
symmetry planes can be defined.  The next “*” card terminates this input.  
  Cards 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
XC1 
YC1 
ZC1 
XC2 
YC2 
ZC2 
Type 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
IDNL 
PID 
Nonlocal material input ID. 
Part ID for nonlocal material. 
P 
Q 
L 
NFREQ 
Exponent  of  weighting  function.    A  typical  value  might  be  8
depending somewhat on the choice of L.  See equations below. 
Exponent  of  weighting  function.    A  typical  value  might  be  2.
See equations below. 
Characteristic  length.    This  length  should  span  a  few  elements. 
See equations below. 
Number  of  time  steps  between  searching  for  integration  points
that lie in the neighborhood.  Nonlocal smoothing will be done
each  cycle  using  these  neighbors  until  the  next  search  is  done.
The neighbor search can add significant computational time so it
is suggested that NFREQ be set to value of 10 to 100 depending
on  the  problem.    This  parameter  may  be  somewhat  problem
dependent.    If  NFREQ = 0,  a  single  search  will  be  done  at  the 
start of the calculation. 
NHV 
Define the number of history variables for nonlocal treatment. 
NL1, …, NL8 
Identifies the history variable(s) for nonlocal treatment.  Define
NHV values (maximum of 8 values per line). 
XC1, YC1, ZC1 
Coordinate of point on symmetry plane. 
XC2, YC2, ZC2 
Coordinate of a point along the normal vector.
*MAT 
For elastoplastic material models in LS-DYNA which  use the plastic strain as a failure 
criterion, setting the variable NL1 to 1  would tag plastic  strain for nonlocal treatment.  
A  sampling  of  other  history  variables  that  can  be  tagged  for  nonlocal  treatment  are 
listed in the table below.  The value in the third column in the table below corresponds 
to the history variable number as tabulated at http://www.dynasupport.com/howtos-
/material/history-variables.    Note  that  the  NLn  value  is  the  history  variable  number 
plus 1. 
Material Model Name 
JOHNSON_COOK 
PLASTICITY_WITH_DAMAGE 
DAMAGE_1 
DAMAGE_2 
JOHNSON_HOLMQUIST_CONCRETE 
GURSON 
15 
81 
104 
105 
111 
120 
*MAT_NONLOCAL 
NLn Value 
History Variable 
Number 
5 (shells); 7 (solids) 
4 (shells); 6 (solids) 
2 
4 
2 
2 
2 
1 
3 
1 
1 
1 
In applying the nonlocal equations to shell and thick shell elements, integration points 
lying  in  the  same  plane  within  the  radius  determined  by  the  characteristic  length  are 
considered.    Therefore,  it  is  important  to  define  the  connectivity  of  the  shell  elements 
consistently within the part ID, e.g., so that the outer integration points lie on the same 
surface. 
The equations and our implementation are based on the implementation by Worswick 
and Lalbin [1999] of the nonlocal theory to Pijaudier-Cabot and Bazant [1987].   Let  Ω𝑟 
be  the  neighborhood  of  radius,  L,  of  element  𝑒𝑟  and  {𝑒𝑖}𝑖=1,...,𝑁𝑟  the  list  of  elements 
included in Ω𝑟, then 
𝑟 = 𝑓 ̇(𝑥𝑟) =
𝑓 ̇
𝑊𝑟
local𝑤(𝑥𝑟 − 𝑦)
∫ 𝑓 ̇
𝛺𝑟
𝑑𝑦 ≈
𝑊𝑟
𝑁𝑟
∑ 𝑓 ̇
𝑖=1
local
𝑤𝑟𝑖
𝑉𝑖 
where 
𝑊𝑟 = 𝑊(𝑥𝑟) = ∫ 𝑤(𝑥𝑟 − 𝑦) 𝑑𝑦 ≈ ∑ 𝑤𝑟𝑖𝑉𝑖
𝑁𝑟
𝑤𝑟𝑖 = 𝑤(𝑥𝑟 − 𝑦𝑖) =
𝑖=1
[1 + (
∥𝑥𝑟 − 𝑦𝑖∥
𝑞 
)
]
Figure  2-3.    Here  𝑓 ̇
𝑟  and  𝑥𝑟  are  respectively  the  nonlocal  rate  of  increase  of
damage  and  the  center  of  the  element 𝑒𝑟,  and  𝑓 ̇
,  𝑉𝑖  and  𝑦𝑖  are  respectively 
local
the local rate of increase of damage, the volume and the center of element 𝑒𝑖.
*MAT_001 
This  is  Material  Type  1.    This  is  an  isotropic  hypoelastic  material  and  is  available  for 
beam,  shell,  and  solid  elements  in  LS-DYNA.    A  specialization  of  this  material  allows 
the modeling of fluids. 
Available options include: 
<BLANK> 
FLUID 
such that the keyword cards appear: 
*MAT_ELASTIC or MAT_001 
*MAT_ELASTIC_FLUID or MAT_001_FLUID 
The fluid option is valid for solid elements only. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
DA 
F 
6 
DB 
F 
7 
K 
F 
8 
Default 
none 
none 
none 
0.0 
0.0 
0.0 
0.0 
Additional card for FLUID keyword option. 
3 
4 
5 
6 
7 
8 
  Card 2 
Variable 
1 
VC 
Type 
F 
2 
CP 
F 
Default 
none  1.0E+20 
  VARIABLE   
MID 
LS-DYNA R10.0 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
*MAT_ELASTIC 
DESCRIPTION
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
Axial  damping  factor (used  for Belytschko-Schwer  beam,  type  2, 
only). 
Bending damping factor (used for Belytschko-Schwer beam, type 
2, only). 
Bulk Modulus (define for fluid option only). 
Tensor  viscosity  coefficient,  values  between  .1  and  .5  should  be
okay. 
Cavitation pressure (default = 1.0e+20). 
RO 
E 
PR 
DA 
DB 
K 
VC 
CP 
Remarks: 
This  hypoelastic  material  model  may  not  be  stable  for  finite  (large)  strains.      If  large 
strains  are  expected,  a  hyperelastic  material  model,  e.g.,  *MAT_002,  would  be  more 
appropriate. 
The axial and bending damping factors are used to damp down numerical noise.  The 
update  of  the  force  resultants,  𝐹𝑖,  and  moment  resultants,  𝑀𝑖,  includes  the  damping 
factors: 
𝑛+1 = 𝐹𝑖
𝐹𝑖
𝑛 + (1 +
𝑛+1
2 
) Δ𝐹𝑖
𝐷𝐴
Δ𝑡
𝑀𝑖
𝑛+1 = 𝑀𝑖
𝑛 + (1 +
𝑛+1
2 
) Δ𝑀𝑖
𝐷𝐵
Δ𝑡
The  history  variable  labeled  as  “plastic  strain”  by  LS-PrePost  is  actually  volumetric 
strain in the case of *MAT_ELASTIC. 
Truss elements include a damping stress given by 
𝜎 = 0.05𝜌𝑐𝐿/𝛥𝑡 
where ρ is the mass density, 𝑐 is the material wave speed, 𝐿 is the element length, and 𝛥𝑡 
is the computation time step.
For the fluid option, the bulk modulus field, 𝐾, must be defined, and both the Young’s 
modulus  and  Poisson’s  ratio  fields  are  ignored.    With  the  fluid  option,  fluid-like 
behavior is obtained where the bulk modulus, 𝐾, and pressure rate, 𝑝, are given by: 
𝐾 =
3(1 − 2𝜈)
𝑝̇ = −𝐾𝜀̇𝑖𝑖 
and  the  shear  modulus  is  set  to  zero.    A  tensor  viscosity  is  used  which  acts  only  the 
𝑛+1, given in terms of the damping coefficient as: 
deviatoric stresses, 𝑆𝑖𝑗
𝑛+1 = VC × Δ𝐿 × 𝑎 × 𝜌𝜀̇𝑖𝑗
′  
𝑆𝑖𝑗
where Δ𝐿 is a characteristic element length, 𝑎 is the fluid bulk sound speed, 𝜌 is the fluid 
density, and 𝜀̇𝑖𝑗
′  is the deviatoric strain rate.
*MAT_OPTIONTROPIC_ELASTIC 
This  is  Material  Type  2.    This  material  is  valid  for  modeling  the  elastic-orthotropic 
behavior of solids, shells, and thick shells.  An anisotropic option is available for solid 
elements.  For orthotropic solids an isotropic frictional damping is available. 
In the case of solids, stresses are calculated not from incremental strains but rather from 
the deformation gradient.  Also for solids, the elastic constants are formulated in terms 
of second Piola-Kirchhoff stress and Green’s strain, however, Cauchy stress is output. 
In  the  case  of  shells,  the  stress  update  is  incremental  and  the  elastic  constants  are 
formulated in terms of Cauchy stress and true strain. 
NOTE: This material does not support specification of a ma-
terial  angle,  𝛽𝑖,  for  each  through-thickness  integra-
tion point of a shell. 
Available options include: 
ORTHO 
ANISO 
such that the keyword cards appear: 
*MAT_ORTHOTROPIC_ELASTIC or MAT_002 
(4 cards follow) 
*MAT_ANISOTROPIC_ELASTIC or MAT_002_ANIS 
(5 cards follow) 
Orthotropic Card 1.  Card 1 for ORTHO keyword option. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
EA 
F 
4 
EB 
F 
5 
EC 
F 
6 
7 
8 
PRBA 
PRCA 
PRCB 
F 
F 
F 
Orthotropic Card 2.  Card 2 for ORTHO keyword option. 
  Card 2 
1 
2 
3 
4 
Variable 
GAB 
GBC 
GCA 
AOPT 
Type 
F 
F 
F 
F 
5 
G 
F 
6 
7 
8 
SIGF
Anisotropic Card 1.  Card 1 for ANISO keyword option. 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
4 
5 
6 
7 
8 
C11 
C12 
C22 
C13 
C23 
C33 
Type 
A8 
F 
F 
F 
F 
F 
F 
F 
Anisotropic Card 2.  Card 2 for ANISO keyword option. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
C14 
C24 
C34 
C44 
C15 
C25 
C35 
C45 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Anisotropic Card 3.  Card 3 for ANISO keyword option. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
C55 
C16 
C26 
C36 
C46 
C56 
C66 
AOPT 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Local Coordinate System Card 1.  Required for  all keyword options 
  Card 4 
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
3 
ZP 
F 
4 
A1 
F 
5 
A2 
F 
6 
A3 
F 
7 
8 
MACF 
IHIS 
I
Local Coordinate System Card 2.  Required for  all keyword options 
  Card 5 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
7 
8 
BETA 
REF 
F 
F 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density. 
Define for the ORTHO option only: 
EA 
EB 
EC 
PRBA 
PRCA 
PRCB 
GAB 
GBC 
GCA 
𝐸𝑎, Young’s modulus in 𝑎-direction. 
𝐸𝑏, Young’s modulus in 𝑏-direction. 
𝐸𝑐,  Young’s  modulus  in  𝑐-direction  (nonzero  value  required  but 
not used for shells). 
𝜈𝑏𝑎, Poisson’s ratio in the 𝑏𝑎 direction. 
𝜈𝑐𝑎, Poisson’s ratio in the 𝑐𝑎 direction. 
𝜈𝑐𝑏, Poisson’s ratio in the 𝑐𝑏 direction. 
𝐺𝑎𝑏, shear modulus in the 𝑎𝑏 direction. 
𝐺𝑏𝑐, shear modulus in the 𝑏𝑐 direction. 
𝐺𝑐𝑎, shear modulus in the 𝑐𝑎 direction. 
Due to symmetry define the upper triangular Cij’s for the ANISO option only: 
C11 
C12 
⋮ 
C66 
The  1,  1  term  in  the  6  ×  6  anisotropic  constitutive  matrix.    Note 
that 1 corresponds to the a material direction 
The  1,  2  term  in  the  6  ×  6  anisotropic  constitutive  matrix.    Note 
that 2 corresponds to the b material direction 
The 6, 6 term in the 6 × 6 anisotropic constitutive matrix. 
⋮
Define AOPT for both options: 
AOPT 
Material axes option, see Figure M2-1. 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element  nodes  as  shown  in  part  (a)  of  Figure  M2-1. 
The 𝐚-direction is from node 1 to node 2 of the element.
The  𝐛-direction  is  orthogonal  to  the  a-direction  and  is 
in  the  plane  formed  by  nodes  1,  2,  and  4.    When  this
option is used  in two-dimensional planar and axisym-
metric  analysis,  it  is  critical  that  the  nodes  in  the  ele-
ment definition be numbered counterclockwise for this
option to work correctly. 
EQ.1.0: locally orthotropic with material axes determined by a
point  in  space  and  the  global  location  of  the  element
center;  this  is  the  𝐚-direction.    This  option  is  for  solid 
elements only. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by 
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  𝐯  with  the 
element  normal.    The  plane  of  a  solid  element  is  the
midsurface between the inner surface and outer surface
defined by the first four nodes and the last four nodes
of the connectivity of the element, respectively. 
EQ.4.0: locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector  𝐯,  and 
an originating point, 𝐏, which define the centerline ax-
is.  This option is for solid elements only. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID 
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
G 
Shear  modulus  for  frequency  independent  damping.    Frequency
independent  damping  is  based  of  a  spring  and  slider  in  series.
The critical stress for the slider mechanism is SIGF defined below.
For  the  best  results,  the  value  of  G  should  be  250-1000  times 
greater than SIGF.  This option applies only to solid elements.
SIGF 
Limit stress for frequency independent, frictional, damping. 
XP, YP, ZP 
Define coordinates of point 𝐩 for AOPT = 1 and 4. 
A1, A2, A3 
Define components of vector 𝐚 for AOPT = 2. 
MACF 
Material axes change flag for brick elements: 
EQ.1: No change, default, 
EQ.2: switch material axes 𝑎 and 𝑏, 
EQ.3: switch material axes 𝑎 and 𝑐, 
EQ.4: switch material axes 𝑏 and 𝑐. 
IHIS 
Flag  for  anisotropic  stiffness  terms  initialization  (for  solid
elements only). 
EQ.0: C11, C12, … from Cards 1, 2, and 3 are used. 
EQ.1: C11,  C12,  …  are  initialized  by  *INITIAL_STRESS_SOL-
ID’s history data. 
V1, V2, V3 
Define components of vector 𝐯 for AOPT = 3 and 4. 
D1, D2, D3 
Define components of vector 𝐝 for AOPT = 2. 
BETA 
REF 
Material  angle  in  degrees  for  AOPT = 3,  may  be  overridden  on 
the element card, see *ELEMENT_SHELL_BETA or *ELEMENT_-
SOLID_ORTHO. 
Use  reference  geometry  to  initialize  the  stress  tensor.    The
reference  geometry  is  defined  by  the  keyword:  *INITIAL_-
FOAM_REFERENCE_GEOMETRY . 
EQ.0.0: off, 
EQ.1.0: on. 
Remarks: 
The material law that relates stresses to strains is defined as: 
𝐂 = 𝐓T𝐂𝐿𝐓 
where 𝐓 is a transformation matrix, and 𝐂𝐿 is the constitutive matrix defined in terms of 
the  material  constants  of  the  orthogonal  material  axes,  {𝐚, 𝐛, 𝐜}.    The  inverse  of    𝐂𝐿for 
the orthotropic case is defined as:
−1 =
𝐂𝐿
𝐸𝑎
𝜐𝑎𝑏
𝐸𝑎
𝜐𝑎𝑐
𝐸𝑎
−
−
−
−
𝜐𝑏𝑎
𝐸𝑏
𝐸𝑏
𝜐𝑏𝑐
𝐸𝑏
−
−
𝜐𝑐𝑎
𝐸𝑐
𝜐𝑐𝑏
𝐸𝑐
𝐸𝑐
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
𝐺𝑎𝑏
𝐺𝑏𝑐
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
𝐺𝑐𝑎⎦
where, 
𝜐𝑎𝑏
𝐸𝑎
=
𝜐𝑏𝑎
𝐸𝑏
,
𝜐𝑐𝑎
𝐸𝑐
=
𝜐𝑎𝑐
𝐸𝑎
,
𝜐𝑐𝑏
𝐸𝑐
=
𝜐𝑏𝑐
𝐸𝑏
. 
The frequency independent damping is obtained by having a spring and slider in series 
as shown in the following sketch:  
friction
This  option  applies  only  to  orthotropic  solid  elements  and  affects  only  the  deviatoric 
stresses. 
The  procedure  for  describing  the  principle  material  directions  is  now  explained  for 
solid  and  shell  elements  for  this  material  model  and  other  anisotropic  materials.    We 
will  call  the  material  coordinate  system  the  {𝐚, 𝐛, 𝐜}  coordinate  system.    The  AOPT 
options illustrated in Figure M2-1 define the preliminary {𝐚, 𝐛, 𝐜} system for all elements 
of the parts that use the material, but this is not the final material direction.  The {𝐚, 𝐛, 𝐜} 
system defined by the AOPT options may be offset by a final rotation about the 𝐜-axis.  
The offset angle we call BETA. 
For  solid  elements,  the  BETA  angle  is  specified  in  one  of  two  ways.    When  using 
AOPT = 3,  the  BETA  parameter  defines  the  offset  angle  for  all  elements  that  use  the 
material.    The  BETA  parameter  has  no  meaning  for  the  other  AOPT  options.  
Alternatively, a BETA angle can be defined for individual solid elements as described in 
remark  5  for  *ELEMENT_SOLID_ORTHO.    The  beta  angle  by  the  ORTHO  option  is 
available for all values of AOPT, and it overrides the BETA angle on the *MAT card for 
AOPT = 3. 
The  directions  determined  by  the  material  AOPT  options  may  be  overridden  for 
individual  elements  as  described  in  remark  3  for  *ELEMENT_SOLID_ORTHO.  
However,  be  aware  that  for  materials  with  AOPT = 3,  the  final  {𝐚, 𝐛, 𝐜}  system  will  be
the  system  defined  on  the  element  card  rotated  about  𝐜-axis  by  the  BETA  angle 
specified on the *MAT card. 
There  are  two  fundamental  differences  between  shell  and  solid  element  orthotropic 
materials.    First,  the  𝐜-direction  is  always  normal  to  a  shell  element  such  that  the  𝐚-
direction  and  𝐛-directions  are  within  the  plane  of  the  element.    Second,  for  some 
anisotropic materials, shell elements may have unique fiber directions within each layer 
through the thickness of the element so that a layered composite can be modeled with a 
single element. 
When  AOPT = 0  is  used  in  two-dimensional  planar  and  axisymmetric  analysis,  it  is 
critical that the nodes in the element definition be numbered counterclockwise for this 
option to work correctly. 
Because shell elements have their 𝐜-axes defined by the element normal, AOPT = 1 and 
AOPT = 4  are  not  available  for  shells.    Also,  AOPT = 2  requires  only  the  vector  𝐚  be 
defined since 𝐝 is not used.  The shell procedure projects the inputted 𝐚-direction onto 
each element surface. 
Similar  to  solid  elements,  the  {𝐚, 𝐛, 𝐜}  coordinate  system  determined  by  AOPT  is  then 
modified  by  a  rotation  about  the 𝐜-axis  which  we  will  call  𝜙.    For  those  materials  that 
allow a unique rotation angle for each integration point through the element thickness, 
the rotation angle is calculated by 
𝜙𝑖 = 𝛽 + 𝛽𝑖 
where  𝛽  is  a  rotation  for  the  element,  and  𝛽𝑖  is  the  rotation  for  the  i’th  layer  of  the 
element.  The 𝛽 angle can be input using the BETA parameter on the *MAT data, or will 
be  overridden  for  individual  elements  if  the  BETA  keyword  option  for  *ELEMENT_-
SHELL  is  used.    The  𝛽𝑖  angles  are  input  using  the  ICOMP = 1  option  of  *SECTION_-
SHELL or with *PART_COMPOSITE.  If 𝛽 or 𝛽𝑖 is omitted, they are assumed to be zero. 
All anisotropic shell materials have the BETA parameter on the *MAT card available for 
both  AOPT = 0  and  AOPT = 3,  except  for  materials  91  and  92  which  have  it  available 
(but called FANG instead of BETA) for AOPT = 0, 2, and 3. 
All  anisotropic  shell  materials  allow  an  angle  for  each  integration  point  through  the 
thickness, 𝛽𝑖, except for materials 2, 86, 91, 92, 117, 130, 170, 172, and 194.   
This discussion of material direction angles in shell elements also applies to thick shell 
elements  which  allow  modeling  of  layered  composites  using  *INTEGRATION_SHELL 
or *PART_COMPOSITE_TSHELL.
Illustration of AOPT: Figure M2-1 
AOPT = 0.0 
AOPT = 1.0 (solid only) 
v14
c = a×b
a = v12
b = v14 - a a⋅v14
a⋅a
⇒ a⋅b = 0 
ez
ey
ex
b = c x a  
d ∕∕ ez
c = a x d
a is set parallel to the 
line segment connecting
p to the element center.
d is set parallel to ez.
input(p) → {a} → {c} → {b} 
AOPT = 2.0 (solid) 
AOPT = 2.0 (shell) 
c is orthogonal
to the a,d plane
c = a × d 
a,d are input.
The computed
axes do not
depend on the
element.
b = c × a 
b is orthogonal
to the c,a plane
a = ainput -  
⋅n
ainput
n⋅n
c = n
ainput
b = c×a
AOPT = 3.0 
AOPT = 4.0 (solid only) 
c = n
b = v - c 
c⋅v
c⋅c
a = b×n
b is the projection of v
(from input) onto the
midplane/shell.
Taken together, point
p and vector v define
the axis of symmetry.
a = b×c
b ∕∕ v
c is parallel to the segment
connecting the element
center to the symmetry axis.
(cid:13)(cid:51)(cid:36)(cid:53)(cid:55)
(cid:66)(cid:77)(cid:84)(cid:109)(cid:105)
(cid:98)(cid:118)(cid:75)(cid:35)(cid:81)(cid:72)(cid:103)(cid:47)(cid:50)(cid:98)(cid:43)
(cid:84)(cid:66)(cid:47)
(cid:75)(cid:66)(cid:47)
(cid:99)(cid:51)(cid:106)(cid:99) (cid:66)(cid:47) (cid:56)(cid:82)(cid:97) (cid:106)(cid:64)(cid:67)(cid:99) (cid:85)(cid:29)(cid:97)(cid:106)
(cid:85)(cid:82)(cid:67)(cid:78)(cid:106)(cid:51)(cid:97) (cid:106)(cid:82) (cid:76)(cid:29)(cid:106)(cid:51)(cid:97)(cid:67)(cid:29)(cid:73)
(cid:13)(cid:40)(cid:47)(cid:40)(cid:48)(cid:40)(cid:49)(cid:55)(cid:66)(cid:54)(cid:50)(cid:47)(cid:44)(cid:39)(cid:66)(cid:94)(cid:50)(cid:51)(cid:55)(cid:44)(cid:50)(cid:49)(cid:96)
(cid:66)(cid:77)(cid:84)(cid:109)(cid:105)
(cid:98)(cid:118)(cid:75)(cid:35)(cid:81)(cid:72)(cid:103)(cid:47)(cid:50)(cid:98)(cid:43)
(cid:84)(cid:66)(cid:47)
(cid:35)(cid:50)(cid:105)(cid:28)(cid:103)(cid:28)(cid:83)
(cid:86)(cid:28)(cid:83)(cid:87)(cid:46) (cid:28)(cid:108)(cid:46) (cid:28)(cid:107)
(cid:47)(cid:83)(cid:46) (cid:47)(cid:108)(cid:46) (cid:47)(cid:107)
(cid:85)(cid:82)(cid:67)(cid:78)(cid:106)(cid:51)(cid:97) (cid:106)(cid:82) (cid:85)(cid:29)(cid:97)(cid:106)
(cid:1804)(cid:1397)(cid:46) (cid:48)(cid:51)(cid:56)(cid:29)(cid:110)(cid:73)(cid:106)(cid:99) (cid:106)(cid:82) (cid:122)
(cid:531)(cid:1397)(cid:46) (cid:82)(cid:85)(cid:106)(cid:67)(cid:82)(cid:78)(cid:29)(cid:73)
(cid:534)(cid:1397)(cid:46) (cid:82)(cid:85)(cid:106)(cid:67)(cid:82)(cid:78)(cid:29)(cid:73)
(cid:105)(cid:64)(cid:51)(cid:78) (cid:73)(cid:51)(cid:106)
(cid:531) (cid:30) (cid:531)(cid:1397)
(cid:533) (cid:30) (cid:531)(cid:1397) (cid:3701) (cid:534)(cid:1397)
(cid:532) (cid:30) (cid:533)(cid:1397) (cid:3701) (cid:531)(cid:1397)(cid:15)
(cid:1804)(cid:1397) (cid:67)(cid:99) (cid:78)(cid:82)(cid:106) (cid:48)(cid:51)(cid:126)(cid:78)(cid:51)(cid:48)(cid:89)
(cid:47)(cid:82)(cid:51)(cid:99) (cid:106)(cid:64)(cid:67)(cid:99)
(cid:51)(cid:73)(cid:51)(cid:76)(cid:51)(cid:78)(cid:106) (cid:64)(cid:29)(cid:113)(cid:51)
(cid:531)(cid:1397) (cid:29)(cid:78)(cid:48) (cid:534)(cid:1397)(cid:93)
(cid:119)(cid:51)(cid:99)
(cid:78)(cid:82)
(cid:43)(cid:29)(cid:73)(cid:44)(cid:110)(cid:73)(cid:29)(cid:106)(cid:51) (cid:531)(cid:46) (cid:532)(cid:46) (cid:29)(cid:78)(cid:48) (cid:533) (cid:56)(cid:97)(cid:82)(cid:76)
(cid:544)(cid:1429)(cid:46) (cid:531)(cid:1429)(cid:46) (cid:550)(cid:1429)(cid:46) (cid:29)(cid:78)(cid:48) (cid:534)(cid:1429) (cid:29)(cid:44)(cid:65)
(cid:44)(cid:82)(cid:97)(cid:48)(cid:67)(cid:78)(cid:60) (cid:106)(cid:82) (cid:28)(cid:81)(cid:84)(cid:105) (cid:86)(cid:99)(cid:51)(cid:51)
(cid:28)(cid:81)(cid:84)(cid:105) (cid:126)(cid:60)(cid:110)(cid:97)(cid:51)(cid:87)(cid:89)
(cid:13)(cid:48)(cid:36)(cid:55)
(cid:66)(cid:77)(cid:84)(cid:109)(cid:105)
(cid:98)(cid:118)(cid:75)(cid:35)(cid:81)(cid:72)(cid:103)(cid:47)(cid:50)(cid:98)(cid:43)
(cid:99)(cid:51)(cid:106) (cid:66)(cid:47) (cid:56)(cid:82)(cid:97) (cid:106)(cid:64)(cid:67)(cid:99) (cid:76)(cid:29)(cid:106)(cid:51)(cid:97)(cid:67)(cid:29)(cid:73)
(cid:29)(cid:117)(cid:51)(cid:99) (cid:29)(cid:73)(cid:60)(cid:82)(cid:97)(cid:67)(cid:106)(cid:64)(cid:76) (cid:127)(cid:29)(cid:60)
(cid:29)(cid:117)(cid:51)(cid:99) (cid:44)(cid:64)(cid:29)(cid:78)(cid:60)(cid:51) (cid:127)(cid:29)(cid:60)
(cid:544)(cid:1429)
(cid:531)(cid:1429)
(cid:550)(cid:1429)
(cid:534)(cid:1429)
(cid:1804)(cid:1429)(cid:46) (cid:48)(cid:51)(cid:56)(cid:29)(cid:110)(cid:73)(cid:106)(cid:99) (cid:106)(cid:82) (cid:122)
(cid:75)(cid:66)(cid:47)
(cid:28)(cid:81)(cid:84)(cid:105)
(cid:75)(cid:28)(cid:43)(cid:55)
(cid:116)(cid:84)(cid:46) (cid:118)(cid:84)(cid:46) (cid:120)(cid:84)
(cid:28)(cid:83)(cid:46) (cid:28)(cid:108)(cid:46) (cid:28)(cid:107)
(cid:112)(cid:83)(cid:46) (cid:112)(cid:108)(cid:46) (cid:112)(cid:107)
(cid:47)(cid:83)(cid:46) (cid:47)(cid:108)(cid:46) (cid:47)(cid:107)
(cid:35)(cid:50)(cid:105)(cid:28)
(cid:119)(cid:51)(cid:99)
(cid:34)(cid:48)(cid:49)(cid:53) (cid:30) (cid:20)(cid:93)
(cid:78)(cid:82)
(cid:96)(cid:82)(cid:106)(cid:29)(cid:106)(cid:51) (cid:531) (cid:29)(cid:78)(cid:48) (cid:532)
(cid:36)(cid:119) (cid:1804)(cid:1429) (cid:29)(cid:36)(cid:82)(cid:110)(cid:106) (cid:533)(cid:89)
(cid:78)(cid:82)
(cid:96)(cid:82)(cid:106)(cid:29)(cid:106)(cid:51) (cid:531) (cid:29)(cid:78)(cid:48) (cid:532)
(cid:36)(cid:119) (cid:1804)(cid:1397) (cid:29)(cid:36)(cid:82)(cid:110)(cid:106) (cid:533)(cid:89)
(cid:1804)(cid:1397) (cid:48)(cid:51)(cid:126)(cid:78)(cid:51)(cid:48)(cid:93)
(cid:119)(cid:51)(cid:99)
(cid:28)(cid:85)(cid:85)(cid:73)(cid:119) (cid:75)(cid:28)(cid:43)(cid:55)(cid:89)
(cid:96)(cid:51)(cid:106)(cid:110)(cid:97)(cid:78) (cid:531)(cid:46)
(cid:532)(cid:46) (cid:29)(cid:78)(cid:48) (cid:533)(cid:89)
(cid:105)(cid:67)(cid:76)(cid:51) (cid:51)(cid:113)(cid:82)(cid:73)(cid:113)(cid:51) (cid:531)(cid:46) (cid:532)(cid:46) (cid:29)(cid:78)(cid:48)
(cid:533) (cid:115)(cid:67)(cid:106)(cid:64) (cid:106)(cid:64)(cid:51) (cid:51)(cid:73)(cid:51)(cid:76)(cid:51)(cid:78)(cid:106)(cid:89)
Figure  M2-2.    Flow  chart  showing  how  for  each  solid  element  LS-DYNA 
determines the vectors {𝒂, 𝒃, 𝒄} from the input.
(cid:13)(cid:54)(cid:40)(cid:38)(cid:55)(cid:44)(cid:50)(cid:49)(cid:66)(cid:54)(cid:43)(cid:40)(cid:47)(cid:47)
(cid:13)(cid:48)(cid:36)(cid:55)
(cid:66)(cid:77)(cid:84)(cid:109)(cid:105)
(cid:98)(cid:118)(cid:75)(cid:35)(cid:81)(cid:72)(cid:103)(cid:47)(cid:50)(cid:98)(cid:43)
(cid:98)(cid:50)(cid:43)(cid:66)(cid:47) (cid:99)(cid:51)(cid:106)(cid:99) (cid:99)(cid:51)(cid:44)(cid:106)(cid:67)(cid:82)(cid:78) (cid:66)(cid:47)
(cid:66)(cid:43)(cid:81)(cid:75)(cid:84)
(cid:98)(cid:98)(cid:35)(cid:83)(cid:46) (cid:98)(cid:98)(cid:35)(cid:108)(cid:46) (cid:15)(cid:15)(cid:15)
(cid:127)(cid:29)(cid:60)(cid:46) (cid:67)(cid:56) (cid:83) (cid:97)(cid:51)(cid:29)(cid:48) (cid:1804)(cid:1413)
(cid:29)(cid:78)(cid:60)(cid:73)(cid:51)(cid:99)(cid:45) (cid:1804)(cid:1413)(cid:46)
(cid:13)(cid:51)(cid:36)(cid:53)(cid:55)
(cid:66)(cid:77)(cid:84)(cid:109)(cid:105)
(cid:98)(cid:118)(cid:75)(cid:35)(cid:81)(cid:72)(cid:103)(cid:47)(cid:50)(cid:98)(cid:43)
(cid:84)(cid:66)(cid:47) (cid:99)(cid:51)(cid:106) (cid:85)(cid:29)(cid:97)(cid:106) (cid:66)(cid:47)
(cid:75)(cid:66)(cid:47) (cid:85)(cid:82)(cid:67)(cid:78)(cid:106)(cid:51)(cid:97) (cid:106)(cid:82) (cid:76)(cid:29)(cid:106)(cid:51)(cid:97)(cid:67)(cid:29)(cid:73)
(cid:98)(cid:50)(cid:43)(cid:66)(cid:47) (cid:85)(cid:82)(cid:67)(cid:78)(cid:106)(cid:51)(cid:97) (cid:106)(cid:82) (cid:99)(cid:51)(cid:44)(cid:106)(cid:67)(cid:82)(cid:78)
(cid:13)(cid:40)(cid:47)(cid:40)(cid:48)(cid:40)(cid:49)(cid:55)(cid:66)(cid:54)(cid:43)(cid:40)(cid:47)(cid:47)(cid:66)(cid:94)(cid:50)(cid:51)(cid:55)(cid:44)(cid:50)(cid:49)(cid:96)
(cid:66)(cid:77)(cid:84)(cid:109)(cid:105)
(cid:98)(cid:118)(cid:75)(cid:35)(cid:81)(cid:72)(cid:103)(cid:47)(cid:50)(cid:98)(cid:43)
(cid:84)(cid:66)(cid:47) (cid:85)(cid:82)(cid:67)(cid:78)(cid:106)(cid:51)(cid:97) (cid:106)(cid:82) (cid:85)(cid:29)(cid:97)(cid:106)
(cid:75)(cid:43)(cid:66)(cid:47) (cid:85)(cid:82)(cid:67)(cid:78)(cid:106)(cid:51)(cid:97) (cid:106)(cid:82) (cid:44)(cid:82)(cid:82)(cid:97)(cid:48)(cid:67)(cid:78)(cid:29)(cid:106)(cid:51) (cid:99)(cid:119)(cid:99)(cid:106)(cid:51)(cid:76)
(cid:35)(cid:50)(cid:105)(cid:28) (cid:1804)(cid:1397)(cid:46) (cid:48)(cid:51)(cid:56)(cid:29)(cid:110)(cid:73)(cid:106)(cid:99) (cid:106)(cid:82) (cid:122)
(cid:66)(cid:77)(cid:84)(cid:109)(cid:105)
(cid:98)(cid:118)(cid:75)(cid:35)(cid:81)(cid:72)(cid:103)(cid:47)(cid:50)(cid:98)(cid:43)
(cid:75)(cid:66)(cid:47) (cid:99)(cid:51)(cid:106)(cid:99) (cid:76)(cid:29)(cid:106)(cid:51)(cid:97)(cid:67)(cid:29)(cid:73) (cid:66)(cid:47)
(cid:28)(cid:81)(cid:84)(cid:105)
(cid:28)(cid:83)(cid:46) (cid:28)(cid:108)(cid:46) (cid:28)(cid:107)
(cid:112)(cid:83)(cid:46) (cid:112)(cid:108)(cid:46) (cid:112)(cid:107)
(cid:29)(cid:117)(cid:51)(cid:99) (cid:29)(cid:73)(cid:60)(cid:82)(cid:97)(cid:67)(cid:106)(cid:64)(cid:76) (cid:127)(cid:29)(cid:60)
(cid:531)(cid:1429)
(cid:550)(cid:1429)
(cid:35)(cid:50)(cid:105)(cid:28) (cid:1804)(cid:1429)(cid:46) (cid:48)(cid:51)(cid:56)(cid:29)(cid:110)(cid:73)(cid:106)(cid:99) (cid:106)(cid:82) (cid:122)
(cid:13)(cid:51)(cid:36)(cid:53)(cid:55)(cid:66)(cid:38)(cid:50)(cid:48)(cid:51)(cid:50)(cid:54)(cid:44)(cid:55)(cid:40)
(cid:66)(cid:77)(cid:84)(cid:109)(cid:105)
(cid:98)(cid:118)(cid:75)(cid:35)(cid:81)(cid:72)(cid:103)(cid:47)(cid:50)(cid:98)(cid:43)
(cid:84)(cid:66)(cid:47) (cid:99)(cid:51)(cid:106)(cid:99) (cid:85)(cid:29)(cid:97)(cid:106) (cid:66)(cid:47)
(cid:75)(cid:66)(cid:47)(cid:83)(cid:46) (cid:75)(cid:66)(cid:47)(cid:108)(cid:46) (cid:89)(cid:89)(cid:89)
(cid:84)(cid:43)(cid:35)(cid:83)(cid:46) (cid:84)(cid:43)(cid:35)(cid:108)(cid:46) (cid:89)(cid:89)(cid:89)
(cid:85)(cid:82)(cid:67)(cid:78)(cid:106)(cid:51)(cid:97) (cid:106)(cid:82) (cid:76)(cid:29)(cid:106)(cid:51)(cid:97)(cid:67)(cid:29)(cid:73)
(cid:29)(cid:78)(cid:60)(cid:73)(cid:51)(cid:99)(cid:45) (cid:1804)(cid:1413)
(cid:11)(cid:36)(cid:12)
(cid:119)(cid:51)(cid:99)
(cid:66)(cid:99) (cid:75)(cid:43)(cid:66)(cid:47)
(cid:48)(cid:51)(cid:126)(cid:78)(cid:51)(cid:48)(cid:93)
(cid:78)(cid:82)
(cid:98)(cid:51)(cid:106) (cid:531)(cid:46) (cid:532)(cid:46) (cid:29)(cid:78)(cid:48)
(cid:533) (cid:56)(cid:97)(cid:82)(cid:76) (cid:44)(cid:82)(cid:82)(cid:97)(cid:65)
(cid:48)(cid:67)(cid:78)(cid:29)(cid:106)(cid:51) (cid:99)(cid:119)(cid:99)(cid:106)(cid:51)(cid:76)
(cid:75)(cid:43)(cid:66)(cid:47)(cid:89)
(cid:66)(cid:99) (cid:84)(cid:66)(cid:47) (cid:29)
(cid:44)(cid:82)(cid:76)(cid:85)(cid:82)(cid:99)(cid:67)(cid:106)(cid:51)(cid:93)
(cid:11)(cid:37)(cid:12)
(cid:11)(cid:38)(cid:12)
(cid:119)(cid:51)(cid:99)
(cid:77) (cid:53) (cid:83)
(cid:75) (cid:53) (cid:75)(cid:66)(cid:47)(cid:77)
(cid:86)(cid:56)(cid:97)(cid:82)(cid:76) (cid:44)(cid:82)(cid:76)(cid:85)(cid:82)(cid:99)(cid:67)(cid:106)(cid:51)(cid:87)
(cid:77) (cid:2957) (cid:77) (cid:90) (cid:83)
(cid:78)(cid:82)
(cid:75) (cid:53) (cid:75)(cid:66)(cid:47)
(cid:86)(cid:56)(cid:97)(cid:82)(cid:76) (cid:84)(cid:28)(cid:96)(cid:105)(cid:87)
(cid:78)(cid:82)
(cid:43)(cid:29)(cid:73)(cid:44)(cid:110)(cid:73)(cid:29)(cid:106)(cid:51) (cid:531)(cid:46) (cid:532)(cid:46) (cid:29)(cid:78)(cid:48) (cid:533) (cid:56)(cid:97)(cid:82)(cid:76) (cid:531)(cid:1429)
(cid:29)(cid:78)(cid:48) (cid:550)(cid:1429) (cid:29)(cid:44)(cid:44)(cid:82)(cid:97)(cid:48)(cid:67)(cid:78)(cid:60) (cid:106)(cid:82) (cid:28)(cid:81)(cid:84)(cid:105) (cid:56)(cid:82)(cid:97)
(cid:76)(cid:29)(cid:106)(cid:51)(cid:97)(cid:67)(cid:29)(cid:73) (cid:75) (cid:86)(cid:99)(cid:51)(cid:51) (cid:28)(cid:81)(cid:84)(cid:105) (cid:126)(cid:60)(cid:110)(cid:97)(cid:51)(cid:87)(cid:89)
(cid:66)(cid:99) (cid:76)(cid:29)(cid:106)(cid:51)(cid:97)(cid:67)(cid:29)(cid:73) (cid:75)
(cid:29)(cid:78)(cid:67)(cid:99)(cid:82)(cid:106)(cid:97)(cid:82)(cid:85)(cid:67)(cid:44)(cid:93)
(cid:119)(cid:51)(cid:99)
(cid:28)(cid:81)(cid:84)(cid:105) (cid:67)(cid:99)
(cid:51)(cid:67)(cid:106)(cid:64)(cid:51)(cid:97) (cid:122) (cid:82)(cid:97) (cid:107)(cid:93)
(cid:119)(cid:51)(cid:99)
(cid:1804)(cid:1397) (cid:48)(cid:51)(cid:126)(cid:78)(cid:51)(cid:48)(cid:93)
(cid:119)(cid:51)(cid:99)
(cid:1804) (cid:53) (cid:1804)(cid:1397)
(cid:1804) (cid:53) (cid:1804)(cid:1429)
(cid:78)(cid:82)
(cid:96)(cid:82)(cid:106)(cid:29)(cid:106)(cid:51) (cid:531) (cid:29)(cid:78)(cid:48)
(cid:532) (cid:36)(cid:119) (cid:1804) (cid:29)(cid:36)(cid:82)(cid:110)(cid:106)
(cid:533)(cid:89)
(cid:78)(cid:82)
(cid:72)(cid:51)(cid:106) (cid:1804)(cid:1429) (cid:30) (cid:17)
(cid:11)(cid:39)(cid:12)
(cid:98)(cid:51)(cid:106) (cid:29)(cid:73)(cid:73)
(cid:92)(cid:1804)(cid:94)(cid:1413) (cid:30) (cid:17)
(cid:92)(cid:1804)(cid:1413)(cid:94) (cid:30) (cid:92)(cid:458)(cid:445)(cid:444)(cid:451)(cid:94)
(cid:92)(cid:1804)(cid:1413)(cid:94) (cid:30) (cid:92)(cid:461)(cid:461)(cid:444)(cid:451)(cid:94)
(cid:119)(cid:51)(cid:99)
(cid:119)(cid:51)(cid:99)
(cid:66)(cid:99) (cid:84)(cid:66)(cid:47) (cid:29)
(cid:44)(cid:82)(cid:76)(cid:85)(cid:82)(cid:99)(cid:67)(cid:106)(cid:51)(cid:93)
(cid:78)(cid:82)
(cid:66)(cid:43)(cid:81)(cid:75)(cid:84) (cid:53) (cid:83)(cid:93)
(cid:78)(cid:82)
(cid:105)(cid:67)(cid:76)(cid:51) (cid:51)(cid:113)(cid:82)(cid:73)(cid:113)(cid:51) (cid:531)(cid:46)
(cid:532)(cid:46) (cid:533)(cid:46) (cid:29)(cid:78)(cid:48) (cid:92)(cid:1804)(cid:1413)(cid:94)(cid:89)
(cid:96)(cid:51)(cid:106)(cid:110)(cid:97)(cid:78) (cid:531)(cid:46) (cid:532)(cid:46)
(cid:533)(cid:46) (cid:29)(cid:78)(cid:48) (cid:92)(cid:1804)(cid:1413)(cid:94)(cid:89)
Figure  M2-3.    Flowchart  for  shells:  (a)  check  for  coordinate  system  ID;  (b)
process AOPT; (c) deterimine 𝛽; and (d) for each layer determine 𝛽𝑖.
*MAT_003 
This  is  Material  Type  3.    This  model  is  suited  to  model  isotropic  and  kinematic 
hardening plasticity with the option of including rate effects.  It is a very cost effective 
model and is available for beam (Hughes-Liu and Truss), shell, and solid elements. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
6 
7 
8 
SIGY 
ETAN 
BETA 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
0.0 
0.0 
5 
6 
7 
8 
  Card 2 
1 
2 
Variable 
SRC 
SRP 
Type 
F 
F 
3 
FS 
F 
4 
VP 
F 
Default 
0.0 
0.0 
1.E+20 
0.0 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
SIGY 
ETAN 
BETA 
SRC 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
Yield stress. 
Tangent modulus, see Figure M3-1 
Hardening parameter, 0 < 𝛽′ < 1.  See comments below. 
Strain rate parameter, C, for Cowper Symonds strain rate model,
see below.  If zero, rate effects are not considered..
Et
Yield
Stress
⎛
⎜
⎝
⎛
⎜
⎝
l0
ln
β=0, kinematic hardening
β=1, isotropic hardening
Figure M3-1.  Elastic-plastic behavior with kinematic and isotropic hardening
where  𝑙0  and  𝑙  are  undeformed  and  deformed  lengths  of  uniaxial  tension
specimen.  𝐸𝑡 is the slope of the bilinear stress strain curve. 
  VARIABLE   
DESCRIPTION
Strain rate parameter, P, for Cowper Symonds strain rate model,
see below.  If zero, rate effects are not considered. 
Effective plastic strain for eroding elements. 
Formulation for rate effects: 
EQ.0.0: Scale yield stress (default), 
EQ.1.0: Viscoplastic formulation (recommended) 
SRP 
FS 
VP 
Remarks: 
Strain  rate  is  accounted  for  using  the  Cowper  and  Symonds  model  which  scales  the 
yield stress with the factor 
1  +   (
𝜀̇
𝑝⁄
)
where  𝜀̇  is  the  strain  rate.    A  fully  viscoplastic  formulation  is  optional  which 
incorporates the Cowper and Symonds formulation within the yield surface.  To ignore 
strain rate effects set both SRC and SRP to zero. 
Kinematic,  isotropic,  or  a  combination  of  kinematic  and  isotropic  hardening  may  be 
specified by varying 𝛽′ between 0 and 1.  For 𝛽′ equal to 0 and 1, respectively, kinematic
and  isotropic  hardening  are  obtained  as  shown  in  Figure  M3-1.    For  isotropic 
hardening, 𝛽′= 1, Material Model 12, *MAT_ISOTROPIC_ELASTIC_PLASTIC, requires 
less storage and is more efficient.  Whenever possible, Material 12 is recommended for 
solid  elements,  but  for  shell  elements  it  is  less  accurate  and  thus  Material  12  is  not 
recommended in this case.
*MAT_ELASTIC_PLASTIC_THERMAL 
This  is  Material  Type  4.    Temperature  dependent  material  coefficients  can  be  defined.  
A  maximum  of  eight  temperatures  with  the  corresponding  data  can  be  defined.    A 
minimum  of  two  points  is  needed.    When  this  material  type  is  used  it  is  necessary  to 
define nodal temperatures by activating a coupled analysis or by using another option 
to  define  the  temperatures  such  as  *LOAD_THERMAL_LOAD_CURVE,  or  *LOAD_-
THERMAL_VARIABLE. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
  Card 2 
Variable 
1 
T1 
Type 
F 
  Card 3 
Variable 
1 
E1 
Type 
F 
  Card 4 
1 
2 
T2 
F 
2 
E2 
F 
2 
3 
4 
5 
6 
7 
8 
3 
T3 
F 
3 
E3 
F 
3 
4 
T4 
F 
4 
E4 
F 
4 
5 
T5 
F 
5 
E5 
F 
5 
6 
T6 
F 
6 
E6 
F 
6 
7 
T7 
F 
7 
E7 
F 
7 
8 
T8 
F 
8 
E8 
F 
8 
Variable 
PR1 
PR2 
PR3 
PR4 
PR5 
PR6 
PR7 
PR8 
Type 
F 
F 
F 
F 
F 
F 
F
No defaults are assumed.  
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ALPHA1 
ALPHA2 
ALPHA3 
ALPHA4 
ALPHA5 
ALPHA6 
ALPHA7 
ALPHA8 
Type 
F 
  Card 6 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
SIGY1 
SIGY2 
SIGY3 
SIGY4 
SIGY5 
SIGY6 
SIGY7 
SIGY8 
Type 
F 
  Card 7 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
ETAN1 
ETAN2 
ETAN3 
ETAN4 
ETAN5 
ETAN6 
ETAN7 
ETAN8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
TI 
EI 
PRI 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Temperatures.  The minimum is 2, the maximum is 8. 
Corresponding Young’s moduli at temperature TI. 
Corresponding Poisson’s ratios. 
ALPHAI 
Corresponding coefficients of thermal expansion. 
SIGYI 
Corresponding yield stresses. 
ETANI 
Corresponding plastic hardening moduli.
*MAT_ELASTIC_PLASTIC_THERMAL 
The  stress  update  for  this  material  follows  the  standard  approach  to  hypo-
elastoplasticity, using Jaumann rate for objectivity.  The rate of Cauchy stress 𝝈 can in 
principal be expressed as 
𝝈̇ = 𝑪(𝜺̇ − 𝜺̇𝑇 − 𝜺̇𝑝) + 𝑪̇𝑪−1𝝈 
where  𝑪  is  the  temperature  dependent  isotropic  elasticity  tensor,  𝜺̇  is  the  rate-of-
deformation, 𝜺̇𝑇 is the thermal strain rate and 𝜺̇𝑝 is the plastic strain rate.  The coefficient 
of  thermal  expansion  is  defined  as  the  instantaneous  value.    Thus,  the  thermal  strain 
rate becomes 
𝜺̇𝑇 = 𝛼𝑇̇𝑰 
where  𝛼  is  the  temperature  dependent  thermal  expansion  coefficient,  𝑇̇  is  the  rate  of 
temperature  and  𝑰  is  the  identity  tensor.    Associated  von  Mises  plasticity  is  adopted, 
resulting in  
𝜺̇𝑝 = 𝜀̇𝑝
3𝒔
2𝜎̅̅̅̅̅
where 𝜀̇𝑝 is the effective plastic strain rate, 𝒔 is the deviatoric stress tensor and 𝜎̅̅̅̅̅ is the 
von  Mises  effective  stress.    The  last  term  accounts  for  stress  changes  due  to  change  in 
stiffness with respect to temperature, using the total elastic strain defined as 𝜺𝑒 = 𝑪−1𝝈.  
A  way  to  intuitively  understand  this  contribution,  for  small  displacement  elasticity  if 
neglecting everything but the temperature dependent elasticity parameters, we have 
𝝈̇ =
𝑑𝑡
(𝑪𝜺) 
as a special case, showing that the stress may change without any change in strain. 
At least two temperatures and their corresponding material properties must be defined.  
The analysis will be terminated if a material temperature falls outside the range defined 
in the input.  If a thermo-elastic material is considered, do not define SIGY and ETAN.
*MAT_005 
This  is  Material  Type  5.    It  is  a  relatively  simple  material  model  for  representing  soil, 
concrete, or crushable foam.  A table can be defined if thermal effects are considered in 
the pressure versus volumetric strain behavior.   
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
G 
F 
3 
4 
KUN 
F 
4 
5 
A0 
F 
5 
6 
A1 
F 
6 
7 
A2 
F 
7 
8 
PC 
F 
8 
Variable 
VCR 
REF 
LCID 
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
4 
5 
6 
7 
8 
Variable 
EPS1 
EPS2 
EPS3 
EPS4 
EPS5 
EPS6 
EPS7 
EPS8 
Type 
F 
  Card 4 
1 
F 
2 
Variable 
EPS9 
EPS10 
Type 
F 
F 
  Card 5 
Variable 
1 
P1 
Type 
F 
2 
P2 
F 
F 
3 
3 
P3 
F 
F 
4 
4 
P4 
F 
F 
5 
5 
P5 
F 
F 
6 
6 
P6 
F 
F 
7 
7 
P7 
F 
F 
8 
8 
P8
4 
5 
6 
7 
8 
*MAT_005 
  Card 6 
Variable 
1 
P9 
2 
P10 
Type 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
G 
Material identification.  A unique number or label not exceeding
8 characters must be specified. 
Mass density. 
Shear modulus. 
KUN 
Bulk modulus for unloading used for VCR = 0.0. 
A0 
A1 
A2 
PC 
Yield function constant for plastic yield function below. 
Yield function constant for plastic yield function below. 
Yield function constant for plastic yield function below. 
Pressure cutoff for tensile fracture (< 0). 
VCR 
Volumetric crushing option: 
EQ.0.0: on, 
EQ.1.0: loading and unloading paths are the same. 
REF 
Use  reference  geometry  to  initialize  the  pressure.    The  reference
geometry  is  defined  by  the  keyword:*INITIAL_FOAM_REFER-
ENCE_GEOMETRY. 
the
deviatoric stress state. 
  This  option  does  not 
initialize 
EQ.0.0: off, 
EQ.1.0: on.
VARIABLE   
LCID 
EPS1, … 
DESCRIPTION
Load  curve  ID  for  compressive  pressure  (ordinate)  as  a  function
of volumetric strain (abscissa).  If LCID is defined, then the curve
is  used  instead  of  the  input  for  EPS1…,  and  P1….    It  makes  no
difference  whether  the  values  of  volumetric  strain  in  the  curve 
are input as positive or negative since internally, a negative sign
is  applied  to  the  absolute  value  of  each  abscissa  entry.    The
response  is  extended  to  being  temperature  dependent  if  LCID
refers to a table. 
Volumetric strain values in pressure vs.  volumetric strain curve 
.  A maximum of 10 values including 0.0 are
allowed and a minimum of 2 values are necessary.  If EPS1 is not
0.0  then  a  point  (0.0, 0.0)  will  be  automatically  generated  and  a 
maximum of nine values may be input. 
P1, P2, …, PN 
Pressures  corresponding  to  volumetric  strain  values  given  on
Cards 3 and 4.
Loading and unloading (along the grey
arows) follows the input curve when the
volumetric crushing option is off (VCR = 1.0)
tension
Pressure Cutoff Value
compression
Volumetric Strain,
ln
⎛
⎜
⎝
⎛
⎜
⎝
V0
The bulk unloading modulus is used
if the volumetric crushing option is on 
(VCR = 0).  In thiscase the aterial's response
follows the black arrows.
Figure  M5-1.    Pressure  versus  volumetric  strain  curve  for  soil  and  crushable
foam  model.    The  volumetric  strain  is  given  by  the  natural  logarithm  of  the
relative volume, 𝑉. 
Remarks: 
Pressure is positive in compression.  Volumetric strain is given by the natural log of the 
relative  volume  and  is  negative  in  compression.    Relative  volume  is  a  ratio  of  the 
current volume to the initial volume at the start of the calculation.  The tabulated data 
should  be  given  in  order  of  increasing  compression.    If  the  pressure  drops  below  the 
cutoff  value  specified,  it  is  reset  to  that  value.    For  a  detailed  description  we  refer  to 
Kreig [1972]. 
The  deviatoric  perfectly  plastic  yield  function,  𝜙,  is  described  in  terms  of  the  second 
invariant 𝐽2, 
𝐽2    =   
 𝑠𝑖𝑗𝑠𝑖𝑗, 
pressure, 𝑝, and constants 𝑎0, 𝑎1, and 𝑎2 as: 
𝜙 = 𝐽2 − [𝑎0 + 𝑎1𝑝 + 𝑎2𝑝2]. 
On the yield surface 𝐽2 = 1
3 𝜎𝑦
2 where 𝜎𝑦 is the uniaxial yield stress, i.e., 
there is no strain hardening on this surface.   
𝜎𝑦 = [3(𝑎0 + 𝑎1𝑝 + 𝑎2𝑝2)]
2⁄
To eliminate the pressure dependence of the yield strength, set: 
𝑎1 = 𝑎2 = 0   and   𝑎0 =
2. 
𝜎𝑦
This approach is useful when a von Mises type elastic-plastic model is desired for use 
with the tabulated volumetric data. 
The  history  variable  labeled  as  “plastic  strain”  by  LS-PrePost  is  actually  plastic 
volumetric strain.  Note that when VCR = 1.0, plastic volumetric strain is zero.
*MAT_VISCOELASTIC 
This  is  Material  Type  6.    This  model  allows  the  modeling  of  viscoelastic  behavior  for 
beams  (Hughes-Liu),  shells,  and  solids.    Also  see  *MAT_GENERAL_VISCOELASTIC 
for a more general formulation. 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
BULK 
Type 
A8 
F 
F 
6 
7 
8 
BETA 
F 
4 
G0 
F 
5 
GI 
F 
DESCRIPTION
  VARIABLE   
MID 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density 
BULK 
Elastic bulk modulus. 
LT.0.0: |BULK| is load curve of bulk modulus as a function of
temperature. 
G0 
Short-time shear modulus, see equations below. 
LT.0.0: |G0|  is  load  curve  of  short-time  shear  modulus  as  a 
function of temperature. 
GI 
Long-time (infinite) shear modulus, G∞. 
LT.0.0: |GI|  is  load  curve  of  long-time  shear  modulus  as  a 
function of temperature. 
BETA 
Decay constant. 
LT.0.0: |BETA| is load curve of decay constant as a function of
temperature. 
Remarks: 
The shear relaxation behavior is described by [Hermann and Peterson, 1968]: 
A Jaumann rate formulation is used 
𝐺(𝑡) = 𝐺∞ + (𝐺0 − 𝐺∞)exp (−𝛽𝑡)
∇
′ = 2 ∫ 𝐺(𝑡 − 𝜏)𝐷′𝑖𝑗(𝜏)𝑑𝜏
ij
∇
𝑖𝑗, and the strain rate, D𝑖𝑗.
where the prime denotes the deviatoric part of the stress rate, 𝜎
*MAT_BLATZ-KO_RUBBER 
This  is  Material  Type  7.    This  one  parameter  material  allows  the  modeling  of  nearly 
incompressible continuum rubber.  The Poisson’s ratio is fixed to 0.463. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
G 
F 
4 
REF 
F 
5 
6 
7 
8 
  VARIABLE   
DESCRIPTION
MID 
RO 
G 
REF 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Shear modulus. 
Use  reference  geometry  to  initialize  the  stress  tensor.    The
reference geometry is defined by the keyword:*INITIAL_FOAM_-
REFERENCE_GEOMETRY . 
EQ.0.0: off, 
EQ.1.0: on. 
Remarks: 
The strain energy density potential for the Blatz-Ko rubber is 
𝑊(𝐂) =
[𝐼1 − 3 +
−𝛽 − 1)] 
(𝐼3
where  𝐺  is  the  shear  modulus,  𝐼1  and  𝐼3  are  the  first  and  third  invariants  of  the  right 
Cauchy-Green tensor 𝐂 = 𝐅T𝐅 and 
1 − 2𝑣
The second Piola-Kirchhoff stress is computed as 
𝛽 =
. 
𝐒 = 2
𝜕𝑊
𝜕𝐂
= 𝐺[𝐈 − 𝐼3
−𝛽𝐂−1] 
from  which  the  Cauchy  stress  is  obtained  by  a  push-forward  from  the  reference  to 
current configuration divided by the relative volume 𝐽 = det(𝑭),
𝛔 =
𝐅𝐒𝐅T =
[𝐁 − 𝐼3
−𝛽𝐈]. 
Here we used 𝐁 = 𝐅𝐅T to denote the left Cauchy-Green tensor, and the Poisson ratio 𝑣 
above is set internally to 𝑣 = 0.463, also see Blatz and Ko [1962].
*MAT_HIGH_EXPLOSIVE_BURN 
This is Material Type 8.  It allows the modeling of the detonation of a high explosive.  In 
addition an equation of state must be defined.  See Wilkins [1969] and Giroux [1973]. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
D 
F 
4 
5 
PCJ 
BETA 
F 
F 
6 
K 
F 
7 
G 
F 
8 
SIGY 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
D 
PCJ 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Detonation velocity. 
Chapman-Jouget pressure. 
BETA 
Beta burn flag, BETA : 
EQ.0.0: beta and programmed burn, 
EQ.1.0: beta burn only, 
EQ.2.0: programmed burn only. 
K 
G 
Bulk modulus (BETA = 2.0 only). 
Shear modulus (BETA = 2.0 only). 
SIGY 
𝜎y, yield stress (BETA = 2.0 only). 
Remarks: 
Burn fractions, 𝐹, which multiply the equations of states for high explosives, control the 
release  of  chemical  energy  for  simulating  detonations.    At  any  time,  the  pressure  in  a 
high explosive element is given by: 
where 𝑝eos, is the pressure from the equation of state (either types 2, 3, or 14), V  is the 
relative volume, and E  is the internal energy density per unit initial volume. 
𝑝 = 𝐹𝑝eos(𝑉, 𝐸)
In the initialization phase, a lighting time tl  is computed for each element by dividing 
the  distance  from  the  detonation  point  to  the  center  of  the  element  by  the  detonation 
velocity  D.    If  multiple  detonation  points  are  defined,  the  closest  detonation  point 
determines tl.  The burn fraction 𝐹 is taken as the maximum 
Where 
𝐹 = max(𝐹1, 𝐹2) 
𝐹1 =
⎧2  (𝑡 − 𝑡𝑙)𝐷𝐴𝑒max
{
3𝑣𝑒  
⎨
{
 0
⎩
if  𝑡  >   𝑡𝑙
if  𝑡  ≤   𝑡𝑙
𝐹2 = 𝛽 =  
1 − 𝑉
1 − 𝑉𝐶𝐽
where 𝑉𝐶𝐽 is the Chapman-Jouguet relative volume and t is current time.  If 𝐹 exceeds 1, 
it is reset to 1.  This calculation of the burn fraction usually requires several time steps 
for  𝐹  to  reach  unity,  thereby  spreading  the  burn  front  over  several  elements.    After 
reaching  unity, 𝐹  is  held  constant.    This  burn  fraction  calculation  is  based  on  work  by 
Wilkins [1964] and is also discussed by Giroux [1973]. 
If  the  beta  burn  option  is  used,  BETA = 1.0,  any  volumetric  compression  will  cause 
detonation and  
and 𝐹1 is not computed. 
𝐹 = 𝐹2 
If programmed burn is used, BETA = 2.0, the undetonated high explosive material will 
behave as an elastic perfectly plastic material if the bulk modulus, shear modulus, and 
yield  stress  are  defined.    Therefore,  with  this  option  the  explosive  material  can 
compress without causing detonation.  The location and time of detonation is controlled 
by *INITIAL_DETONATION. 
As an option, the high explosive material can behave as an elastic perfectly-plastic solid 
prior  to  detonation.    In  this  case  we  update  the  stress  tensor,  to  an  elastic  trial  stress, 
∗ 𝑠𝑖𝑗
𝑛+1, 
∗ 𝑠𝑖𝑗
𝑛+1 = 𝑠𝑖𝑗
𝑛 + 𝑠𝑖𝑝𝛺𝑝𝑗 + 𝑠𝑗𝑝𝛺𝑝𝑖 + 2𝐺𝜀′̇
𝑖𝑗𝑑𝑡 
where 𝐺 is the shear modulus, and 𝜀′̇
condition is given by: 
𝑖𝑗 is the deviatoric strain rate.  The von Mises yield 
𝜙 = 𝐽2 −
𝜎𝑦
where  the  second  stress  invariant,  𝐽2,  is  defined  in  terms  of  the  deviatoric  stress 
components as
and the yield stress is 𝜎𝑦.  If yielding has occurred, i.e., 𝜑 > 0, the deviatoric trial stress 
is scaled to obtain the final deviatoric stress at time n+1: 
𝑠𝑖𝑗𝑠𝑖𝑗 
𝐽2 =
If 𝜑 ≤ 0, then 
𝑛+1 =
𝑠𝑖𝑗
𝜎𝑦
√3𝐽2
∗ 𝑠𝑖𝑗
𝑛+1 
𝑛+1 =∗ 𝑠𝑖𝑗
𝑠𝑖𝑗
𝑛+1 
Before detonation pressure is given by the expression 
𝑝𝑛+1 = Κ (
𝑉𝑛+1 − 1) 
where K is the bulk modulus.  Once the explosive material detonates: 
and the material behaves like a gas.
𝑛+1 = 0 
𝑠𝑖𝑗
This is Material Type 9.  
*MAT_009 
In  the  case  of  solids  and  thick  shells,  this  material  allows  equations  of  state  to  be 
considered  without  computing  deviatoric  stresses.    Optionally,  a  viscosity  can  be 
defined.  Also, erosion in tension and compression is possible. 
Beams  and  shells  that  use  this  material  type  are  completely  bypassed  in  the  element 
processing;  however,  the  mass  of  the  null  beam  or  shell  elements  is  computed  and 
added  to  the  nodal  points  which  define  the  connectivity.    The  mass  of  null  beams  is 
ignored  if  the  value  of  the  density  is  less  than  1.e-11.    The  Young’s  modulus  and 
Poisson’s ratio are used only for setting the contact stiffness, and it is recommended that 
reasonable values be input.  The variables PC, MU, TEROD, and EDROD do not apply 
to beams and shells.  Historically, null beams and/or null shells have been used as an 
aid in modeling of contact but this practice is now seldom needed. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
PC 
F 
4 
5 
6 
7 
MU 
TEROD 
CEROD 
YM 
F 
F 
F 
F 
8 
PR 
F 
Defaults 
none 
none 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
MID 
RO 
PC 
MU 
TEROD 
CEROD 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Pressure cutoff (≤ 0.0).  See Remark 4. 
Dynamic viscosity μ (optional).  See Remark 1. 
Relative volume.  𝑉
𝑉0
greater than unity.  If zero, erosion in tension is inactive. 
, for erosion in tension.  Typically, use values 
Relative  volume,  𝑉
𝑉0
values less than unity.  If zero, erosion in compression is inactive.
,  for  erosion  in  compression.    Typically,  use 
YM 
Young’s modulus (used for null beams and shells only)
*MAT_NULL 
DESCRIPTION
PR 
Poisson’s ratio (used for null beams and shells only) 
Remarks: 
These remarks apply to solids and thick shells only. 
1.  When  used  with  solids  or  thick  shells,  this  material  must  be  used  with  an 
equation-of-state.  Pressure cutoff is negative in tension.  A (deviatoric) viscous 
stress of the form 
𝜎′𝑖𝑗 = 2𝜇𝜀′̇
𝑚2 𝑠] [
𝑚2] ~ [
is computed for nonzero 𝜇 where 𝜀′̇
𝑖𝑗 is the deviatoric strain rate.  𝜇 is the dy-
namic viscosity.  For example, in SI unit system, 𝜇 may have a unit of [Pa*s]. 
𝑖𝑗 
] 
[
2.  Null  material  has  no  shear  stiffness  (except  from  viscosity)  and  hourglass 
control  must  be  used  with  great  care.    In  some  applications,  the  default  hour-
glass coefficient may lead to significant energy losses.  In general for fluid, the 
hourglass coefficient QM should be small (in the range 1.0E-6 to 1.0E-4) and the 
hourglass type IHQ should be set to 1 (default). 
3.  The Null material has no yield strength and behaves in a fluid-like manner. 
4.  The cut-off pressure, PC, must be defined to allow for a material to “numerical-
ly”  cavitate.   In  other words,  when  a  material  undergoes  dilatation  above  cer-
tain  magnitude,  it  should  no  longer  be  able  to  resist  this  dilatation.    Since 
dilatation stress or pressure is negative, setting PC limit to a very small negative 
number would allow for the material to cavitate once the pressure in the mate-
rial goes below this negative value.
*MAT_ELASTIC_PLASTIC_HYDRO_{OPTION} 
This  is  Material  Type  10.    This  material  allows  the  modeling  of  an  elastic-plastic 
hydrodynamic material and requires an equation-of-state (*EOS). 
Available options include: 
<BLANK> 
SPALL 
STOCHASTIC 
The keyword card can appear in two ways: 
*MAT_ELASTIC_PLASTIC_HYDRO or MAT_010 
*MAT_ELASTIC_PLASTIC_HYDRO_SPALL or MAT_010_SPALL 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
G 
F 
4 
SIG0 
F 
5 
EH 
F 
Default 
none 
none 
none 
0.0 
0.0 
6 
PC 
F 
-∞ 
7 
FS 
F 
8 
CHARL 
F 
0.0 
0.0 
Spall Card.  Additional card for SPALL keyword option. 
 Optional 
Variable 
1 
A1 
Type 
F 
  Card 2 
1 
2 
A2 
F 
2 
3 
4 
5 
6 
7 
8 
SPALL 
F 
3 
4 
5 
6 
7 
8 
Variable 
EPS1 
EPS2 
EPS3 
EPS4 
EPS5 
EPS6 
EPS7 
EPS8 
Type 
F 
F 
F 
F 
F 
F 
F
Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EPS9 
EPS10 
EPS11 
EPS12 
EPS13 
EPS14 
EPS15 
EPS16 
Type 
F 
  Card 4 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
ES1 
ES2 
ES3 
ES4 
ES5 
ES6 
ES7 
ES8 
Type 
F 
  Card 5 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
ES9 
ES10 
ES11 
ES12 
ES13 
ES14 
ES15 
ES16 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
G 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Shear modulus. 
SIG0 
Yield stress, see comment below. 
EH 
PC 
FS 
Plastic hardening modulus, see definition below. 
Pressure cutoff (≤ 0.0).  If zero, a cutoff of -∞ is assumed. 
Effective plastic strain at which erosion occurs.
Piecewise linear curve defining
the yield stress versus effective
plastic strain.  As illustrated, the
yield stress at zero plastic strain
should be nonzero.
ep
Figure  M10-1.    Effective  stress  versus  effective  plastic  strain  curve.    See  EPS
and ES input.  
  VARIABLE   
CHARL 
DESCRIPTION
Characteristic  element  thickness  for  deletion.    This  applies  to  2D
solid  elements  that  lie  on  a  boundary of  a  part.   If  the  boundary
element  thins  down  due  to  stretching  or  compression,  and  if  it
thins  to  a  value  less  than  CHARL,  the  element  will  be  deleted. 
The primary application of this option is to  predict the break-up 
of axisymmetric shaped charge jets. 
A1 
A2 
Linear pressure hardening coefficient. 
Quadratic pressure hardening coefficient. 
SPALL 
Spall type: 
EQ.0.0: default set to “1.0”, 
EQ.1.0: tensile pressure is limited by PC, i.e., p is always ≥ PC, 
EQ.2.0: if  𝜎max ≥ −PC  element  spalls  and  tension,  𝑝 < 0,  is 
never allowed, 
EQ.3.0: 𝑝 < PC  element  spalls  and  tension,  𝑝 < 0,  is  never 
allowed. 
EPS 
Effective plastic strain (True).  Define up to 16 values.  Care must
be  taken  that  the  full  range  of  strains  expected  in  the  analysis  is
covered.    Linear extrapolation  is  used  if  the  strain  values  exceed
the maximum input value.   
ES 
Effective stress.  Define up to 16 values.
*MAT_ELASTIC_PLASTIC_HYDRO 
If ES and EPS are undefined, the yield stress and plastic hardening modulus are taken 
from  SIG0  and  EH.    In  this  case,  the  bilinear  stress-strain  curve  shown  in  M10-1  is 
obtained with hardening parameter, 𝛽 = 1.  The yield strength is calculated as 
𝜎𝑦 = 𝜎0 + 𝐸ℎ𝜀̅𝑝 + (𝑎1 + 𝑝𝑎2)max[𝑝, 0] 
The quantity 𝐸ℎ is the plastic hardening modulus defined in terms of Young’s modulus, 
𝐸, and the tangent modulus, 𝐸𝑡, as follows 
and 𝑝 is the pressure taken as positive in compression. 
𝐸ℎ =
𝐸𝑡𝐸
𝐸 − 𝐸𝑡
. 
If ES and EPS are specified, a curve like that shown in M10-1 may be defined.  Effective 
stress is defined in terms of the deviatoric stress tensor, 𝑠𝑖𝑗, as: 
𝜎̅̅̅̅̅ = (
2⁄
𝑠𝑖𝑗𝑠𝑖𝑗)
and effective plastic strain by: 
𝜀̅𝑝 = ∫ (
2⁄
𝑝 )
𝑝 𝐷𝑖𝑗
𝐷𝑖𝑗
𝑑𝑡,
𝑝 is the plastic component of the rate of deformation tensor.  
where t denotes time and 𝐷𝑖𝑗
In this case the plastic hardening modulus on Card 1 is ignored and the yield stress is 
given as 
where the value for 𝑓 (𝜀̅𝑝) is found by interpolation from the data curve. 
𝜎𝑦 = 𝑓 (𝜀̅𝑝), 
A  choice  of  three  spall  models  is  offered  to  represent  material  splitting,  cracking,  and 
failure under tensile loads.  The pressure limit model, SPALL = 1, limits the hydrostatic 
tension  to  the  specified  value,  𝑝cut.    If  pressures  more  tensile  than  this  limit  are 
calculated, the pressure is reset to pcut.  This option is not strictly a spall  model, since 
the deviatoric stresses are unaffected by the pressure reaching the tensile cutoff, and the 
pressure cutoff value, pcut, remains unchanged throughout the analysis. 
The  maximum  principal  stress  spall  model,  SPALL = 2,  detects  spall  if  the  maximum 
principal  stress,  𝜎max,  exceeds  the  limiting  value  -𝑝cut.    Note  that  the  negative  sign  is 
required  because  𝑝cut  is  measured  positive  in  compression,  while  𝜎max  is  positive  in 
tension.  Once spall is detected with this model, the deviatoric stresses are reset to zero, 
and no hydrostatic tension (𝑝 < 0) is permitted.  If tensile pressures are calculated, they
are reset to 0 in the spalled material.  Thus, the spalled material behaves as a rubble or 
incohesive material. 
The  hydrostatic  tension  spall  model,  SPALL = 3,  detects  spall  if  the  pressure  becomes 
more tensile than the specified limit, 𝑝cut.  Once spall is detected the deviatoric stresses 
are  reset  to  zero,  and  nonzero  values  of  pressure  are  required  to  be  compressive 
(positive).  If hydrostatic tension (𝑝 < 0) is subsequently calculated, the pressure is reset 
to 0 for that element. 
This  model  is  applicable  to  a  wide  range  of  materials,  including  those  with  pressure-
dependent  yield  behavior.    The  use  of  16  points  in  the  yield  stress  versus  effective 
plastic  strain  curve  allows  complex  post-yield  hardening  behavior  to  be  accurately 
represented.    In  addition,  the  incorporation  of  an  equation  of  state  permits  accurate 
modeling  of  a  variety  of  different  materials.    The  spall  model  options  permit 
incorporation of material failure, fracture, and disintegration effects under tensile loads. 
The STOCHASTIC option allows spatially varying yield and failure behavior.  See *DE-
FINE_STOCHASTIC_VARIATION for additional information.
*MAT_STEINBERG 
This is Material Type 11.  This material is available for modeling materials deforming at 
very high strain rates (> 105) and can be used with solid elements.  The yield strength is 
a function of temperature and pressure.  An equation of state determines the pressure. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
  Card 2 
Variable 
Type 
  Card 3 
Variable 
1 
B 
F 
1 
PC 
Type 
F 
  Card 4 
1 
2 
BP 
F 
2 
SPALL 
F 
2 
3 
G0 
F 
3 
H 
F 
3 
RP 
F 
3 
7 
8 
GAMA 
SIGM 
4 
5 
SIGO 
BETA 
F 
4 
F 
F 
4 
F 
5 
A 
F 
5 
6 
N 
F 
6 
F 
7 
TMO 
GAMO 
F 
6 
F 
7 
F 
8 
SA 
F 
8 
FLAG 
MMN 
MMX 
ECO 
EC1 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
EC2 
EC3 
EC4 
EC5 
EC6 
EC7 
EC8 
EC9 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
G0 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Basic shear modulus.
VARIABLE   
DESCRIPTION
SIGO 
BETA 
σo, see defining equations. 
β, see defining equations. 
N 
n, see defining equations. 
GAMA 
SIGM 
B 
BP 
H 
F 
A 
γi, initial plastic strain, see defining equations. 
σm, see defining equations.
b, see defining equations. 
b′, see defining equations. 
h, see defining equations. 
f, see defining equations. 
Atomic weight (if = 0.0, R′ must be defined). 
TMO 
Tmo, see defining equations. 
GAMO 
γo, see defining equations. 
SA 
PC 
a, see defining equations. 
Pressure cutoff (default = -1.e+30) 
SPALL 
Spall type: 
EQ.0.0:  default set to “2.0”, 
EQ.1.0:  p ≥ PC, 
EQ.2.0:  if  σmax  ≥  -PC  element  spalls  and  tension,  p < 0,  is 
never allowed, 
EQ.3.0:  p < PC  element  spalls  and  tension,  p < 0,  is  never 
allowed. 
R′.  If R′≠0.0, A is not defined. 
Set  to  1.0  for  μ coefficients  for  the  cold  compression  energy  fit.
Default is η. 
RP 
FLAG 
MMN 
μmin or ηmin.  Optional μ or η minimum value.
*MAT_STEINBERG 
DESCRIPTION
MMX 
μmax or ηmax.  Optional μ or η maximum value. 
EC0, …, EC9 
Cold compression energy coefficients (optional). 
Remarks: 
Users  who  have  an  interest  in  this  model  are  encouraged  to  study  the  paper  by 
Steinberg and Guinan which provides the theoretical basis.  Another useful reference is 
the KOVEC user’s manual. 
In terms of the foregoing input parameters, we define the shear modulus, 𝐺, before the 
material melts as: 
𝐺 = 𝐺0 [1 + 𝑏𝑝𝑉
3⁄ − ℎ (
𝐸𝑖 − 𝐸𝑐
3𝑅′
− 300)] 𝑒
−𝑓 𝐸𝑖
𝐸𝑚−𝐸𝑖 
where 𝑝 is the pressure, 𝑉 is the relative volume, 𝐸𝑐 is the cold compression energy: 
𝐸𝑐(𝑥) = ∫ 𝑝𝑑𝑥
−
900𝑅′exp(𝑎𝑥)
(1 − 𝑥)2(𝛾0−𝑎−1
2⁄ )
, 
𝑥 = 1 − 𝑉, 
and 𝐸𝑚 is the melting energy: 
which is in terms of the melting temperature 𝑇𝑚  (𝑥): 
𝐸𝑚(𝑥) = 𝐸𝑐(𝑥) + 3𝑅′𝑇𝑚(𝑥) 
𝑇𝑚(𝑥) =
𝑇𝑚𝑜exp(2𝑎𝑥)
𝑉2(𝛾𝑜−𝑎−1
3⁄ )
and the melting temperature at 𝜌 = 𝜌𝑜, 𝑇𝑚𝑜. 
In the above equation 𝑅′ is defined by  
𝑅′ =
𝑅𝜌
where 𝑅 is the gas constant and A is the atomic weight.  If 𝑅 is not defined, LS-DYNA 
computes it with 𝑅 in the cm-gram-microsecond system of units. 
The yield strength σy is given by: 
𝜎𝑦 = 𝜎0
′ [1 + 𝑏′𝑝𝑉
3⁄ − ℎ (
𝐸𝑖 − 𝐸𝑐
3𝑅′
− 300)] 𝑒
−𝑓 𝐸𝑖
𝐸𝑚−𝐸𝑖 
if 𝐸𝑚 exceeds 𝐸𝑖.  Here, 𝜎0
′  is given by: 
𝜎0
′ = 𝜎0[1 + 𝛽(𝛾𝑖 + 𝜀̅𝑝)]𝑛
where 0 is the initial yield stress and 𝑖 is the initial plastic strain.  If the work-hardened 
 is set equal to 𝑚.  After the materials melt, 𝜎𝑦 and 𝐺 are 
yield stress 𝜎0
set to one half their initial value. 
′  exceeds 𝑚, 𝜎0
′
If  the  coefficients  EC0,  …,  EC9  are  not  defined  above,  LS-DYNA  will  fit  the  cold 
compression energy to a ten term polynomial  expansion either as a function of μ or η 
depending on the input variable, FLAG, as: 
𝐸𝑐(𝜂𝑖) = ∑ 𝐸𝐶𝑖𝜂𝑖
𝑖=0
𝐸𝑐(𝜇𝑖) = ∑ 𝐸𝐶𝑖𝜇𝑖
𝑖=0
where ECi is the ith coefficient and: 
𝜂 =
𝜌𝑜
𝜇 =
𝜌𝑜
− 1 
A linear least squares method is used to perform the fit. 
A  choice  of  three  spall  models  is  offered  to  represent  material  splitting,  cracking,  and 
failure under tensile loads.  The pressure limit model, SPALL = 1, limits the hydrostatic 
tension  to  the  specified  value,  pcut.    If  pressures  more  tensile  than  this  limit  are 
calculated, the pressure is reset to pcut.  This option is not strictly a spall  model, since 
the deviatoric stresses are unaffected by the pressure reaching the tensile cutoff, and the 
pressure cutoff value, pcut, remains unchanged throughout the analysis.  The maximum 
principal  stress  spall  model,  SPALL = 2,  detects  spall  if  the  maximum  principal  stress, 
σmax, exceeds the limiting value -pcut.  Note that the negative sign is required because 
pcut is measured positive in compression, while σmax is positive in tension.  Once spall 
is detected with this model, the deviatoric stresses are reset to zero, and no hydrostatic 
tension (p < 0) is permitted.  If tensile pressures are calculated, they are reset to 0 in the 
spalled material.  Thus, the spalled material behaves as a rubble or incohesive material.  
The  hydrostatic  tension  spall  model,  SPALL = 3,  detects  spall  if  the  pressure  becomes 
more tensile than the specified limit, pcut.  Once spall is detected the deviatoric stresses 
are  reset  to  zero,  and  nonzero  values  of  pressure  are  required  to  be  compressive 
(positive).  If hydrostatic tension (p < 0) is subsequently calculated, the pressure is reset 
to 0 for that element. 
This  model  is  applicable  to  a  wide  range  of  materials,  including  those  with  pressure-
dependent yield behavior.  In addition, the incorporation of an equation of state permits 
accurate  modeling  of  a  variety  of  different  materials.    The  spall  model  options  permit 
incorporation of material failure, fracture, and disintegration effects under tensile loads.
*MAT_STEINBERG_LUND 
This is Material Type 11.  This material is a modification of the Steinberg model above 
to  include  the  rate  model  of  Steinberg  and  Lund  [1989].    An  equation  of  state 
determines the pressure. 
The keyword cards can appear in two ways: 
*MAT_STEINBERG_LUND or MAT_011_LUND 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
  Card 2 
Variable 
Type 
  Card 3 
Variable 
1 
B 
F 
1 
PC 
Type 
F 
  Card 4 
1 
2 
BP 
F 
2 
SPALL 
F 
2 
3 
G0 
F 
3 
H 
F 
3 
RP 
F 
3 
7 
8 
GAMA 
SIGM 
4 
5 
SIGO 
BETA 
F 
4 
F 
F 
4 
F 
5 
A 
F 
5 
6 
N 
F 
6 
F 
7 
TMO 
GAMO 
F 
6 
F 
7 
F 
8 
SA 
F 
8 
FLAG 
MMN 
MMX 
ECO 
EC1 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
EC2 
EC3 
EC4 
EC5 
EC6 
EC7 
EC8 
EC9 
Type 
F 
F 
F 
F 
F 
F 
F
Card 5 
Variable 
1 
UK 
Type 
F 
2 
C1 
F 
3 
C2 
F 
4 
YP 
F 
5 
YA 
F 
6 
YM 
F 
7 
8 
  VARIABLE   
DESCRIPTION
MID 
RO 
G0 
SIGO 
BETA 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Basic shear modulus. 
σo, see defining equations. 
β, see defining equations. 
N 
n, see defining equations. 
GAMA 
SIGM 
B 
BP 
H 
F 
A 
γi, initial plastic strain, see defining equations. 
σm, see defining equations. 
b, see defining equations. 
b′, see defining equations. 
h, see defining equations. 
f, see defining equations. 
Atomic weight (if = 0.0, R′ must be defined). 
TMO 
Tmo, see defining equations. 
GAMO 
γo, see defining equations. 
SA 
PC 
a, see defining equations. 
pcut or -σf (default = -1.e+30)
VARIABLE   
DESCRIPTION
SPALL 
Spall type: 
EQ.0.0: default set to “2.0”, 
EQ.1.0: p ≥ pmin, 
EQ.2.0: if  𝜎max ≥ −pmin  element  spalls  and  tension,  p < 0,  is 
never allowed, 
EQ.3.0: p < −pmin  element  spalls  and  tension,  p < 0,  is  never 
allowed. 
R′.  If R′≠0.0, A is not defined. 
Set  to  1.0  for  μ  coefficients  for  the  cold  compression  energy  fit.
Default is η. 
μmin or ηmin.  Optional μ or η minimum value. 
μmax or ηmax.  Optional μ or η maximum value. 
RP 
FLAG 
MMN 
MMX 
EC0, …, EC9 
Cold compression energy coefficients (optional). 
UK 
C1 
C2 
YP 
YA 
Activation energy for rate dependent model. 
Exponent prefactor in rate dependent model. 
Coefficient of drag term in rate dependent model. 
Peierls stress for rate dependent model. 
A thermal yield stress for rate dependent model. 
YMAX 
Work hardening maximum for rate model. 
Remarks: 
This model is similar in theory to the *MAT_STEINBERG above but with the addition 
of rate effects.  When rate effects are included, the yield stress is given by: 
𝜎𝑦 = {𝑌𝑇(𝜀̇𝑝, 𝑇) + 𝑌𝐴𝑓 (𝜀𝑝)}
𝐺(𝑝, 𝑇)
𝐺0
There are two imposed limits on the yield stress.  The first is on the thermal yield stress: 
𝑌𝐴𝑓 (𝜀𝑝) = 𝑌𝐴[1 + 𝛽(𝛾𝑖 + 𝜀𝑝)]𝑛 ≤ 𝑌max 
and the second is on the thermal part:
𝑌𝑇 ≤ 𝑌𝑃 
R' is the heat capacity per unit volume.  Most handbooks give the heat capacity per unit 
mass or per mole.  To obtain R', multiply the heat capacity per unit mass by the initial 
density, and to obtain R' from the heat capacity per mole, divide it by the mass per mole 
and then multiply the result by the initial density.  The mass per mole in grams equals 
the atomic weight.  
For example, the heat capacity per mole for aluminum is 24.2 J/mole/K, the density is 
2.70 g/cc,  and  the  atomic  weight  is  13.    The  heat  capacity  per  cubic  centimeter  is 
therefore  (24.2  J/mole/K) /  (13g/mole) ×  (2.70g/cc)=  5.026  J/cc/K.    To  convert  it  to 
J/m3/K,  multiply  the  result  by  106 cc/m3  to  obtain  a  final  heat  capacity  of  5.026e6 
J/m3/K.
*MAT_ISOTROPIC_ELASTIC_PLASTIC 
This  is  Material  Type  12.    This  is  a  very  low  cost  isotropic  plasticity  model  for  three-
dimensional  solids.    In  the  plane  stress  implementation  for  shell  elements,  a  one-step 
radial return approach is used to scale the Cauchy stress tensor to if the state of stress 
exceeds the yield surface.  This approach to plasticity leads to inaccurate shell thickness 
updates and stresses after yielding.  This is the only model in LS-DYNA for plane stress 
that does not default to an iterative approach. 
Card 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
G 
F 
4 
5 
6 
7 
8 
SIGY 
ETAN 
BULK 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
G 
SIGY 
ETAN 
BULK 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Shear modulus. 
Yield stress. 
Plastic hardening modulus. 
Bulk modulus, K. 
Remarks: 
Here the pressure is integrated in time 
where   𝜀̇𝑖𝑖 is the volumetric strain rate.
𝑝̇ = −𝐾𝜀̇𝑖𝑖
*MAT_ISOTROPIC_ELASTIC_FAILURE 
This  is  Material  Type  13.    This  is  a  non-iterative  plasticity  with  simple  plastic  strain 
failure model. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
G 
F 
4 
5 
6 
7 
8 
SIGY 
ETAN 
BULK 
F 
F 
F 
Default 
none 
none 
none 
none 
0.0 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EPF 
PRF 
REM 
TREM 
Type 
F 
F 
F 
F 
Default 
none 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
MID 
RO 
G 
SIGY 
ETAN 
BULK 
EPF 
PRF 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Shear modulus. 
Yield stress. 
Plastic hardening modulus. 
Bulk modulus. 
Plastic failure strain. 
Failure pressure (≤ 0.0).
*MAT_ISOTROPIC_ELASTIC_FAILURE 
DESCRIPTION
REM 
Element erosion option: 
EQ.0.0:  failed element eroded after failure, 
NE.0.0:  element is kept, no removal except by Δt below. 
TREM 
Δt for element removal: 
EQ.0.0:  Δt is not considered (default), 
GT.0.0:  element eroded if element time step size falls below Δt.
Remarks: 
When the effective plastic strain reaches the failure strain or when the pressure reaches 
the  failure  pressure,  the  element  loses  its  ability  to  carry  tension  and  the  deviatoric 
stresses are set to zero, i.e., the material behaves like a fluid.  If Δt for element removal is 
defined the element removal option is ignored. 
The  element  erosion  option  based  on  Δt  must  be  used  cautiously  with  the  contact 
options.    Nodes  to  surface  contact  is  recommended  with  all  nodes  of  the  eroded  brick 
elements  included  in  the  node  list.   As the  elements  are  eroded the  mass  remains  and 
continues to interact with the master surface.
*MAT_SOIL_AND_FOAM_FAILURE 
This  is  Material  Type  14.    The  input  for  this  model  is  the  same  as  for  *MATERIAL_-
SOIL_AND_FOAM  (Type  5);  however,  when  the  pressure  reaches  the  tensile  failure 
pressure,  the  element  loses  its  ability  to  carry  tension.    It  should  be  used  only  in 
situations  when  soils  and  foams  are  confined  within  a  structure  or  are  otherwise 
confined by nodal boundary conditions.
*MAT_JOHNSON_COOK_{OPTION} 
Available options include: 
<BLANK> 
STOCHASTIC 
This is Material Type 15.  The Johnson/Cook strain and temperature sensitive plasticity 
is  sometimes  used  for  problems  where  the  strain  rates  vary  over  a  large  range  and 
adiabatic temperature increases due to plastic heating cause material softening.  When 
used  with  solid  elements  this  model  requires  an  equation-of-state.    If  thermal  effects 
and  damage  are  unimportant,  the  much  less  expensive  *MAT_SIMPLIFIED_JOHN-
SON_COOK  model  is  recommended.    The  simplified  model  can  be  used  with  beam 
elements. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
G 
F 
4 
E 
F 
5 
PR 
F 
6 
DTF 
F 
7 
VP 
F 
8 
RATEOP 
F 
Default 
none 
none 
none 
none 
none 
0.0 
0.0 
0.0 
  Card 2 
Variable 
Type 
1 
A 
F 
2 
B 
F 
3 
N 
F 
4 
C 
F 
5 
M 
F 
6 
TM 
F 
7 
TR 
F 
8 
EPS0 
F 
Default 
none 
0.0 
0.0 
0.0 
none 
none 
none 
none
Card 3 
Variable 
1 
CP 
Type 
F 
2 
PC 
F 
3 
SPALL 
F 
4 
IT 
F 
5 
D1 
F 
6 
D2 
F 
7 
D3 
F 
8 
D4 
F 
Default 
none 
0.0 
2.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
D5 
C2/P/XNP 
EROD 
EFMIN 
NUMINT 
Type 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
10-6 
F 
0. 
  VARIABLE   
DESCRIPTION
MID 
RO 
G 
E 
PR 
DTF 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Shear  modulus.    G  and  an  equation-of-state  are  required  for 
element  types  that  use  a  3D  stress  update,  e.g.,  solids,  2D  shell
forms 13-15, tshell forms 3 and 5.   For other element types, G is
ignored, and E and PR must be provided. 
Young’s Modulus . 
Poisson’s ratio . 
Minimum  time  step  size  for  automatic  element  deletion  (shell
elements).    The  element  will  be  deleted  when  the  solution  time
step  size  drops  below  DTF × TSSFAC  where  TSSFAC  is  the  time 
step scale factor defined by *CONTROL_TIMESTEP. 
VP 
Formulation for rate effects: 
EQ.0.0: Scale yield stress (default), 
EQ.1.0: Viscoplastic formulation.
*MAT_JOHNSON_COOK 
DESCRIPTION
RATEOP 
Form of strain-rate term.  RATEOP is ignored if VP = 0. 
EQ.0.0: Log-Linear Johnson-Cook (default), 
EQ.1.0: Log-Quadratic Huh-Kang (2 parameters), 
EQ.2.0: Exponential Allen-Rule-Jones, 
EQ.3.0: Exponential Cowper-Symonds (2 parameters). 
EQ.4.0: Nonlinear rate coefficient (2 parameters). 
A 
B 
N 
C 
M 
TM 
TR 
EPS0 
CP 
PC 
See equations below 
See equations below 
See equations below 
See equations below 
See equations below 
Melt temperature 
Room temperature 
Quasi-static  threshold  strain  rate.    Ideally,  this  value  represents
the  highest  strain  rate  for  which  no  rate  adjustment  to  the  flow
stress is needed, and is input in units of [time]−1.  For example, if 
strain  rate  effects  on  the  flow  stress  first  become  apparent  at
strain  rates  greater  than  10−2s−1  and  the  system  of  units  for  the 
model  input  is  kg,  mm,  ms,  then  EPSO  should  be  set  to  10−5, 
which is 10−2s−1 in units of ms. 
Specific  heat  (superseded  by  heat  capacity  in  *MAT_THER-
MAL_OPTION if a coupled thermal/structural analysis) 
Tensile failure stress or tensile pressure cutoff (PC  <  0.0)
VARIABLE   
DESCRIPTION
SPALL 
Spall type: 
EQ.0.0: default set to “2.0”. 
EQ.1.0: Tensile pressure is limited by PC, i.e., 𝑝 is always ≥ PC.
Shell Element Specific Behavior: 
EQ.2.0: Shell elements are deleted when 𝜎max ≥ −PC. 
EQ.3.0: Shell elements are deleted when 𝑝 < 𝑃𝐶. 
Solid Element Specific Behavior 
EQ.2.0:  For solid elements 𝜎max ≥ −PC resets tensile stresses to 
zero.  Compressive stress are still allowed. 
EQ.3.0:  For  solid  elements  𝑝 < PC  resets  the  pressure  to  zero 
thereby disallowing tensile pressure. 
IT 
Plastic  strain  iteration  option.    This  input  applies  to  solid
elements  only  since  it  is  always  necessary  to  iterate  for  the  shell
element plane stress condition. 
EQ.0.0: no iterations (default), 
EQ.1.0: accurate  iterative  solution  for  plastic  strain.    Much
more expensive than default. 
D1 - D5 
Failure parameters, see equations below.  A negative input of D3
will be converted to its absolute value. 
C2/P/XNP 
Optional strain-rate parameter. 
Field  Var Model 
C2 
P 
XNP
𝐶2  Huh-Kang 
𝑃  Cowper-Symonds 
𝑛′  Nonlinear Rate Coefficient 
These models are documented in the remarks. 
EROD 
Erosion Flag: 
EQ.0.0: default, element erosion allowed. 
NE.0.0:  element  does  not  erode;  deviatoric  stresses  set  to  zero
when element fails. 
EFMIN 
The lower bound for calculated strain at fracture .
NUMINT 
*MAT_JOHNSON_COOK 
DESCRIPTION
Number  of  through  thickness  integration  points  which  must  fail
before the shell element is deleted.  (If zero, all points must fail.) 
Since  nodal  fiber  rotations  limit  strains  at  active  integration
points,  the  default,  which  is  to  require  that  all  integration  points 
fail,  is  not  recommended,  because  elements  undergoing  large
strain are often not deleted using this criterion.  Better results may
be obtained when NUMINT is set to 1 or a number less than one
half of the number of through thickness points. 
For example, if four through thickness points are used, NUMINT
should  not  exceed  2,  even  for  fully  integrated  shells  which  have
16 integration points. 
Remarks: 
Johnson and Cook express the flow stress as 
𝜎𝑦 = (𝐴 + 𝐵𝜀̅𝑝𝑛
)(1 + 𝑐 ln 𝜀̇∗)(1 − 𝑇∗𝑚) 
Where, 
𝐴, 𝐵, 𝑐, 𝑛, and 𝑚 =  input constants 
𝜀̅𝑝 =  effective plastic strain 
𝜀̇∗ =
⎧ ε̅
{{
⎨
{{
⎩
EPS0
̇𝑝
ε̅
EPS0
for VP.EQ.0
(normalized effective total strain-rate)
for VP.EQ. 1
(normalized effective plastic strain rate)
𝑇∗ = homologous temperature =
𝑇 − 𝑇room
𝑇melt − 𝑇room
The quantity 𝑇 − 𝑇room is stored as extra history variable 5. 
Constants for a variety of materials are provided in Johnson and Cook [1983].  A fully 
viscoplastic  formulation  is  optional  (VP)  which  incorporates  the  rate  equations  within 
the yield surface.  An additional cost is incurred but the improvement is that results can 
be dramatic. 
Due to nonlinearity in the dependence of flow stress on plastic strain, an accurate value 
of  the  flow  stress  requires  iteration  for  the  increment  in  plastic  strain.    However,  by 
using a Taylor series expansion with linearization about the current time, we can solve 
for σy with sufficient accuracy to avoid iteration. 
2-136 (EOS)
*MAT_015 
𝜀𝑓 = max([𝐷1 + 𝐷2exp𝐷3𝜎 ∗][1 + 𝐷4ln𝜀̇∗][1 + 𝐷5𝑇∗], EFMIN) 
where σ* is the ratio of pressure divided by effective stress 
Fracture occurs when the damage parameter 
𝜎 ∗ =
𝜎eff
𝐷 = ∑
Δ𝜀𝑝
𝜀𝑓
reaches the value of 1.  𝐷 is stored as extra history variable 4 in shell elements and extra 
history variable 6 in solid elements. 
A  choice  of  three  spall  models  is  offered  to  represent  material  splitting,  cracking,  and 
failure  under  tensile  loads.    The  pressure  limit  model  limits  the  minimum  hydrostatic 
pressure  to  the  specified  value,  𝑝 ≥ 𝑝min.    If  pressures  more  tensile  than  this  limit  are 
calculated, the pressure is reset to 𝑝min.  This option is not strictly a spall model since the 
deviatoric  stresses  are  unaffected  by  the  pressure  reaching  the  tensile  cutoff  and  the 
pressure cutoff value 𝑝min remains unchanged throughout the analysis.  The maximum 
principal stress spall model detects spall if the maximum principal stress, 𝜎max, exceeds 
the  limiting  value  𝜎𝑝.    Once  spall  in  solids  is  detected  with  this  model,  the  deviatoric 
stresses are reset to zero and no hydrostatic tension is permitted.  If tensile pressures are 
calculated, they are reset to 0 in the spalled material.  Thus, the spalled material behaves 
as  rubble.    The  hydrostatic  tension  spall  model  detects  spall  if  the  pressure  becomes 
more  tensile  than  the  specified  limit,  𝑝min.    Once  spall  in  solids  is  detected  with  this 
model,  the  deviatoric  stresses  are  set  to  zero  and  the  pressure  is  required  to  be 
compressive.  If hydrostatic tension is calculated then the pressure is reset to 0 for that 
element. 
In  addition  to  the  above  failure  criterion,  this  material  model  also  supports  a  shell 
element deletion criterion based on the maximum stable time step size for the element, 
Δ𝑡max.  Generally, Δ𝑡max goes down as the element becomes more distorted.  To assure 
stability of time integration, the global LS-DYNA time step is the minimum of the Δ𝑡max 
values  calculated  for  all  elements  in  the  model.    Using this  option allows  the  selective 
deletion  of  elements  whose  time  step  Δ𝑡max  has  fallen  below  the  specified  minimum 
time step, Δ𝑡crit.  Elements which are severely distorted often indicate that material has 
failed and supports little load, but these same elements may have very small time steps 
and therefore control the cost of the analysis.  This option allows these highly distorted 
elements to be deleted from the calculation, and, therefore, the analysis can proceed at a 
larger time step, and, thus, at a reduced cost.  Deleted elements do not carry any load, 
and are deleted from all applicable slide surface definitions.  Clearly, this option must 
be judiciously used to obtain accurate results at a minimum cost.
Material type 15 is applicable to the high rate deformation of many materials including 
most  metals.    Unlike  the  Steinberg-Guinan  model,  the  Johnson-Cook  model  remains 
valid  down  to  lower  strain  rates  and  even  into  the  quasistatic  regime.    Typical 
applications include explosive metal forming, ballistic penetration, and impact. 
Optional Strain Rate Forms: 
The standard Johnson-Cook strain rate term is linear in the logarithm of the strain rate: 
1 + 𝐶 ln 𝜀̇∗ 
Some  additional  data  fitting  capability  can  be  obtained  by  using  the  quadratic  form 
proposed by Huh & Kang [2002]: 
1 + 𝐶 ln 𝜀̇∗ + 𝐶2(ln 𝜀̇∗)2 
Three additional exponential forms are available, one due to Allen, Rule & Jones [1997], 
(𝜀̇∗)𝑐 
the Cowper-Symonds-like [1958] form  
and the nonlinear rate coefficient, 
𝜀̇eff
⎟⎞
𝐶 ⎠
⎜⎛
⎝
1 +
𝑛′
𝑝 )
1 + 𝐶(𝜀eff
ln 𝜀̇∗. 
The four additional rate forms (RATEOP = 1, 2, 3 or 4) are currently available for solid 
& shell elements but only when the viscoplastic rate option is active (VP = 1).  If VP is 
set  to  zero,  RATEOP  is  ignored.    See  Huh  and  Kang  [2002],  Allen,  Rule,  and  Jones 
[1997], and Cowper and Symonds [1958]. 
The STOCHASTIC option allows spatially varying yield and failure behavior.  See *DE-
FINE_STOCHASTIC_VARIATION for additional information.
*MAT_016 
This is Material Type 16.  This model has been used to analyze buried steel reinforced 
concrete structures subjected to impulsive loadings. 
5 
6 
7 
8 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
G 
F 
4 
PR 
F 
Default 
none 
none 
none 
none 
  Card 2 
1 
Variable 
SIGF 
Type 
F 
2 
A0 
F 
3 
A1 
F 
4 
A2 
F 
5 
6 
A0F 
A1F 
F 
F 
7 
B1 
F 
8 
PER 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 3 
Variable 
1 
ER 
2 
3 
4 
5 
6 
7 
8 
PRR 
SIGY 
ETAN 
LCP 
LCR 
Type 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
none 
0.0 
none 
none
Variable 
1 
X1 
Type 
F 
*MAT_PSEUDO_TENSOR 
2 
X2 
F 
3 
X3 
F 
4 
X4 
F 
5 
X5 
F 
6 
X6 
F 
7 
X7 
F 
8 
X8 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 5 
Variable 
1 
X9 
2 
3 
4 
5 
6 
7 
8 
X10 
X11 
X12 
X13 
X14 
X15 
X16 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
YS1 
YS2 
YS3 
YS4 
YS5 
YS6 
YS7 
YS8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 7 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
YS9 
YS10 
YS11 
YS12 
YS13 
YS14 
YS15 
YS16 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none
VARIABLE   
DESCRIPTION
MID 
RO 
G 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Shear modulus. 
Poisson’s ratio. 
SIGF 
Tensile cutoff (maximum principal stress for failure). 
A0 
A1 
A2 
A0F 
A1F 
B1 
PER 
ER 
PRR 
SIGY 
ETAN 
LCP 
LCR 
Xn 
Cohesion. 
Pressure hardening coefficient. 
Pressure hardening coefficient. 
Cohesion for failed material. 
Pressure hardening coefficient for failed material. 
Damage scaling factor (or exponent in Mode II.C). 
Percent reinforcement. 
Elastic modulus for reinforcement. 
Poisson’s ratio for reinforcement. 
Initial yield stress. 
Tangent modulus/plastic hardening modulus. 
Load  curve  ID  giving  rate  sensitivity  for  principal  material,  see
*DEFINE_CURVE. 
Load curve ID giving rate sensitivity for reinforcement, see *DE-
FINE_CURVE. 
Effective  plastic  strain,  damage,  or  pressure.    See  discussion
below. 
YSn 
Yield stress (Mode I) or scale factor (Mode II.B or II.C).
Mohr-Coulomb
Tresca
Friction Angle
Cohesion
Figure M16-1.  Mohr-Coulomb surface with a Tresca Limit. 
Pressure
Remarks: 
This  model  can  be  used  in  two  major  modes  -  a  simple  tabular  pressure-dependent 
yield  surface,  and  a  potentially  complex  model  featuring  two  yield  versus  pressure 
functions  with  the  means  of  migrating  from  one  curve  to  the  other.    For  both  modes, 
load curve LCP is taken to be a strain rate multiplier for the yield strength.  Note that 
this model must be used with equation-of-state type 8, 9 or 11. 
Response Mode I.  Tabulated Yield Stress Versus Pressure 
This  model  is  well  suited  for  implementing  standard  geologic  models  like  the  Mohr-
Coulomb  yield  surface  with  a  Tresca  limit,  as  shown  in  Figure  M16-1.    Examples  of 
converting  conventional  triaxial  compression  data  to  this  type  of  model  are  found  in 
(Desai  and  Siriwardane,  1984).    Note  that  under  conventional  triaxial  compression 
conditions,  the  LS-DYNA  input  corresponds  to  an  ordinate  of  𝜎1 − 𝜎3  rather  than  the 
more  widely  used 
,  where  𝜎1  is  the  maximum  principal  stress  and  𝜎3is  the 
minimum principal stress. 
𝜎1−𝜎3
This  material  combined  with  equation-of-state  type  9  (saturated)  has  been  used  very 
successfully  to  model  ground  shocks  and  soil-structure  interactions  at  pressures  up  to 
100kbars (approximately 1.5 x 106 psi).
Figure M16-2.  Two-curve concrete model with damage and failure  
Pressure
To  invoke  Mode  I  of  this  model,  set  a0,  a1,  a2,  b1,  a0f,  and  a1f  to  zero.    The  tabulated 
values  of  pressure  should  then  be  specified  on  cards  4  and  5,  and  the  corresponding 
values of yield stress should be specified on cards 6 and 7.  The parameters relating to 
reinforcement properties, initial yield stress, and tangent modulus are not used in this 
response mode, and should be set to zero. 
Simple tensile failure 
Note  that  a1f  is  reset  internally  to  1/3  even  though  it  is  input  as  zero;  this  defines  a 
failed material curve of slope 3p, where p denotes pressure (positive in compression).  In 
this case the yield strength is taken from the tabulated yield vs.  pressure curve until the 
maximum  principal  stress  (𝜎1)  in  the  element  exceeds  the  tensile  cutoff  𝜎cut  (input  as 
variable  SIGF).    When  𝜎1 > 𝜎cut  is  detected,  the  yield  strength  is  scaled  back  by  a 
fraction of the distance between the two curves in each of the next 20 time steps so that 
after  those  20  time  steps,    the  yield  strength is  defined  by  the  failure  curve.    The  only 
way to inhibit this feature is to set 𝜎𝑐𝑢𝑡 (SIGF) arbitrarily large. 
Response Mode II.  Two Curve Model with Damage and Failure 
This approach uses two yield versus pressure curves of the form  
𝜎𝑦 = 𝑎0 +
𝑎1 + 𝑎2𝑝
The upper curve is best described as the maximum yield strength curve and the lower 
curve is the failed material curve.  There are a variety of ways of moving between the 
two curves and each is discussed below.
MODE II.  A: Simple tensile failure 
Define a0, a1, a2, a0f and a1f, set b1 to zero, and leave cards 4 through 7 blank.  In this case 
the yield strength is taken from the maximum yield curve until the maximum principal 
stress  (𝜎1)  in  the  element  exceeds  the  tensile  cutoff  (𝜎cut).    When  𝜎1 > 𝜎cut  is  detected, 
the yield strength is scaled back by a fraction of the distance between the two curves in 
each  of  the  next  20  time  steps  so  that  after  those  20  time  steps,    the  yield  strength  is 
defined by the failure curve. 
Mode II.B: Tensile failure plus plastic strain scaling 
Define a0, a1, a2, a0f and a1f, set b1 to zero, and user cards 4 through 7 to define a scale 
factor,  η,  versus  effective  plastic  strain.    LS-DYNA  evaluates  η  at  the  current  effective 
plastic strain and then calculated the yield stress as 
𝜎yield = 𝜎failed + 𝜂(𝜎max − 𝜎failed) 
where 𝜎max and 𝜎failed are found as shown in Figure M16-2.  This yield strength is then 
subject to scaling for tensile failure as described above.  This type of model allows the 
description of a strain hardening or softening material such as concrete. 
Mode II.C: Tensile failure plus damage scaling 
The  change  in  yield  stress  as  a  function  of  plastic  strain  arises  from  the  physical 
mechanisms such as internal cracking, and the extent of this cracking is affected by the 
hydrostatic  pressure  when  the  cracking  occurs.    This  mechanism  gives  rise  to  the 
"confinement"  effect  on  concrete  behavior.    To  account  for  this  phenomenon,  a 
"damage"  function  was  defined  and  incorporated.    This  damage  function  is  given  the 
form: 
𝜀𝑝
𝜆 = ∫ (1 +
𝜎cut
)
−𝑏1
𝑑𝜀𝑝
Define a0, a1, a2, a0f and a1f, and b1.  Cards 4 though 7 now give η as a function of λ and 
scale the yield stress as 
and then apply any tensile failure criteria. 
𝜎yield = 𝜎failed + 𝜂(𝜎max − 𝜎failed) 
Mode II Concrete Model Options 
Material  Type  16  Mode  II  provides  for  the  automatic  internal  generation  of  a  simple 
"generic"  model  from  concrete  if  A0  is  negative  then  SIGF  is  assumed  to  be  the 
′  and  –A0  is  assumed  to  be  a  conversion 
unconfined  concrete  compressive  strength,  𝑓𝑐
factor from LS-DYNA pressure units to psi.  (For example, if the model stress units are 
MPa, A0 should be set to –145.) In this case  the parameter values generated internally 
are
′ = SIGF 
𝑓𝑐
𝜎𝑐𝑢𝑡 = 1.7
′2
⎜⎛ 𝑓𝑐
⎟⎞
−𝐴0⎠
⎝
𝑎0 =
′
𝑓𝑐
𝑎1 =
𝑎2 =
′  
3𝑓𝑐
𝑎0𝑓 = 0 
𝑎1𝑓 = 0.385 
Note that these a0f and a1f defaults will be overridden by non zero entries on Card 3.  If 
plastic strain or damage scaling is desired, Cards 5 through 8 and b1 should be specified 
in the input.  When a0 is input as a negative quantity, the equation-of-state can be given 
as  0  and  a  trilinear  EOS  Type  8  model  will  be  automatically  generated  from  the 
unconfined  compressive  strength  and  Poisson's  ratio.    The  EOS  8  model  is  a  simple 
pressure versus volumetric strain model with no internal energy terms, and should give 
reasonable results for pressures up to 5kbar (approximately 75,000 psi). 
Mixture model 
A  reinforcement  fraction,  𝑓𝑟,  can  be  defined  (indirectly  as  PER/100)  along  with 
properties of the reinforcement material.  The bulk modulus, shear modulus, and yield 
strength  are  then  calculated from a  simple  mixture rule, i.e., for the bulk  modulus the 
rule gives: 
𝐾 = (1 − 𝑓𝑟)𝐾𝑚 + 𝑓𝑟𝐾𝑟 
where 𝐾𝑚  and  𝐾𝑟  are the  bulk  moduli  for  the geologic  material  and  the  reinforcement 
material, respectively.  This  feature should be used with  caution.  It gives an isotropic 
effect  in  the  material  instead  of  the  true  anisotropic  material  behavior.    A  reasonable 
approach  would  be  to  use  the  mixture  elements  only  where  the reinforcing  exists  and 
plain  elements  elsewhere.      When  the  mixture  model  is  being  used,  the  strain  rate 
multiplier for the principal material is taken from load curve N1 and the multiplier for 
the reinforcement is taken from load curve N2. 
A Suggestion 
The  LLNL  DYNA3D  manual  from  1991  [Whirley  and  Hallquist]  suggests  using  the 
damage function (Mode II.C.) in Material Type 16 with the following set of parameters: 
𝑎0 =
𝑎1 =
′
𝑓𝑐
𝑎2 =
𝑎0𝑓 =
′
3𝑓𝑐
′
𝑓𝑐
10
𝑎1𝑓 = 1.5 
𝑏1 = 1.25
*MAT_PSEUDO_TENSOR 
Card 4: 
Card 5: 
Card 6: 
Card 7: 
0.0 
5.17E-04 
8.62E-06 
6.38E-04 
2.15E-05 
7.98E-04 
3.14E-05 
3.95E-04 
9.67E-04 
4.00E-03 
1.41E-03 
4.79E-03 
1.97E-03 
0.909 
2.59E-03 
3.27E-03 
0.309 
0.790 
0.383 
0.086 
0.543 
0.630 
0.247 
0.056 
0.840 
0.469 
0.173 
0.0 
0.975 
1.000 
0.136 
0.114 
This set of parameters should give results consistent with Dilger, Koch, and Kowalczyk, 
[1984] for plane concrete.  It has been successfully used for reinforced structures where 
the reinforcing bars were modeled explicitly with embedded beam and shell elements.  
The  model  does  not  incorporate  the  major  failure  mechanism  -  separation  of  the 
concrete  and  reinforcement  leading  to  catastrophic  loss  of  confinement  pressure.  
However,  experience  indicates  that  this  physical  behavior  will  occur  when  this  model 
shows about 4% strain.
*MAT_017 
This  is  Material  Type  17.    This  material  may  be  used  to  model  brittle  materials  which 
fail due to large tensile stresses. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
6 
SIGY 
ETAN 
F 
F 
7 
FS 
F 
8 
PRF 
F 
Default 
none 
none 
none 
none 
none 
0.0 
none 
0.0 
Optional card for crack propagation to adjacent elements :  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SOFT 
CVELO 
Type 
F 
F 
Default 
1.0 
0.0 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
SIGY 
ETAN 
FS 
PRF 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
Yield stress. 
Plastic hardening modulus. 
Fracture stress. 
Failure or cutoff pressure (≤ 0.0).
SOFT 
*MAT_ORIENTED_CRACK 
DESCRIPTION
Factor  by  which  the  fracture  stress  is  reduced  when  a  crack  is
coming from failed neighboring element.  See remarks. 
CVELO 
Crack propagation velocity.  See remarks. 
Remarks: 
This  is  an  isotropic  elastic-plastic  material  which  includes  a  failure  model  with  an 
oriented crack.  The von Mises yield condition is given by: 
𝜙 = 𝐽2 −
𝜎𝑦
where  the  second  stress  invariant,  𝐽2,  is  defined  in  terms  of  the  deviatoric  stress 
components as 
𝐽2 =
𝑠𝑖𝑗𝑠𝑖𝑗 
and  the  yield  stress,𝜎𝑦,  is  a  function  of  the  effective  plastic  strain,  𝜀eff
hardening modulus, 𝐸𝑝: 
𝑝 ,  and  the  plastic 
The effective plastic strain is defined as: 
𝑝  
𝜎𝑦 = 𝜎0 + 𝐸𝑝𝜀eff
𝑝 = ∫ 𝑑𝜀eff
𝜀eff
where 
𝑝 = √
𝑑𝜀eff
𝑝 
𝑝 𝑑𝜀𝑖𝑗
𝑑𝜀𝑖𝑗
and the plastic tangent modulus is defined in terms of the input tangent modulus, 𝐸𝑡, as 
𝐸𝑝 =
𝐸𝐸𝑡
𝐸 − 𝐸𝑡
Pressure in this model is found from evaluating an equation of state.  A pressure cutoff 
can be defined such that the pressure is not allowed to fall below the cutoff value. 
The  oriented  crack  fracture  model  is  based  on  a  maximum  principal  stress  criterion.  
When the maximum principal stress exceeds the fracture stress, 𝜎𝑓 , the element fails on 
a  plane  perpendicular  to  the  direction  of  the  maximum  principal  stress.    The  normal 
stress  and  the  two  shear  stresses  on  that  plane  are  then  reduced  to  zero.    This  stress 
reduction  is  done  according  to  a  delay  function  that  reduces  the  stresses  gradually  to 
zero over a small number of time steps.  This delay function procedure is used to reduce
Figure M17-1.    Thin  structure  (2  elements  over  thickness)  with  cracks  and
necessary element numbering. 
the  ringing  that  may  otherwise  be  introduced  into  the  system  by  the  sudden  fracture. 
The  number  of  steps  for  stress  reduction  is  20  by  default  (CVELO = 0.0)  or  it  is 
internally computed if CVELO > 0.0 is given: 
where Le is characteristic element length and Δt is time step size. 
𝑛steps = int [
𝐿𝑒
CVELO × 𝛥𝑡
] 
After a tensile fracture, the element will not support tensile stress on the fracture plane, 
but in compression will support both normal and shear stresses.  The orientation of this 
fracture  surface  is  tracked  throughout  the  deformation,  and  is  updated  to  properly 
model finite deformation effects.  If the maximum principal stress subsequently exceeds 
the  fracture  stress  in  another  direction,  the  element  fails  isotropically.    In  this  case  the 
element  completely  loses  its  ability  to  support  any  shear  stress  or  hydrostatic  tension, 
and only compressive hydrostatic stress states are possible.  Thus, once isotropic failure 
has occurred, the material behaves like a fluid. 
This model is applicable to elastic or elastoplastic materials under significant tensile or 
shear loading when fracture is expected.  Potential applications include brittle materials 
such  as  ceramics  as  well  as  porous  materials  such  as  concrete  in  cases  where  pressure 
hardening effects are not significant. 
Crack propagation behavior to adjacent elements can be controlled via parameter SOFT 
for thin, shell-like structures (e.g.  only 2 or 3 solids over thickness).  Additionally, LS-
DYNA  has  to  know  where  the  plane  or  solid  element  midplane  is  at  each  integration 
point  for  projection  of  crack  plane  on  this  element  midplane.    Therefore,  element 
numbering has to be as shown in Figure M17-1.  Only solid element type 1 is supported 
with that option at the moment.
*MAT_POWER_LAW_PLASTICITY 
This  is  Material  Type  18.    This  is  an  isotropic  plasticity  model  with  rate  effects  which 
uses a power law hardening rule. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
K 
F 
6 
N 
F 
7 
8 
SRC 
SRP 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
0.0 
0.0 
  Card 2 
1 
Variable 
SIGY 
Type 
F 
2 
VP 
F 
3 
4 
5 
6 
7 
8 
EPSF 
F 
Default 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
K 
N 
SRC 
SRP 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
Strength coefficient. 
Hardening exponent. 
Strain rate parameter, 𝐶, if zero, rate effects are ignored. 
Strain rate parameter, 𝑃, if zero, rate effects are ignored.
VARIABLE   
SIGY 
DESCRIPTION
Optional  input  parameter  for  defining  the  initial  yield  stress,  𝜎𝑦.
Generally, this parameter is not necessary and the strain to yield
is calculated as described below. 
LT.0.02:  𝜀𝑦𝑝 = SIGY 
GT.0.02:  See below. 
Plastic failure strain for element deletion. 
Formulation for rate effects: 
EQ.0.0: Scale yield stress (default), 
EQ.1.0: Viscoplastic formulation. 
EPSF 
VP 
Remarks: 
Elastoplastic  behavior  with  isotropic  hardening  is  provided  by  this  model.    The  yield 
stress, 𝜎𝑦, is a function of plastic strain and obeys the equation: 
𝜎𝑦 = 𝑘𝜀𝑛 = 𝑘(𝜀𝑦𝑝 + 𝜀̅𝑝)
where 𝜀𝑦𝑝 is the elastic strain to yield and 𝜀̅𝑝is the effective plastic strain (logarithmic).  
If  SIGY  is  set  to  zero, the  strain  to yield  if  found  by  solving  for the  intersection  of  the 
linearly elastic loading equation with the strain hardening equation: 
𝜎 = 𝐸𝜀 
𝜎 = 𝑘  𝜀𝑛 
which gives the elastic strain at yield as: 
If SIGY is nonzero and greater than 0.02 then: 
𝜀𝑦𝑝 = (
[ 1
]
𝑛−1
)
𝜀𝑦𝑝 = (
[1
𝑛]
)
𝜎𝑦
Strain  rate  is  accounted  for  using  the  Cowper  and  Symonds  model  which  scales  the 
yield stress with the factor 
1 + (
𝑝⁄
)
𝜀̇
where  𝜀̇  is  the  strain  rate.    A  fully  viscoplastic  formulation  is  optional  which 
incorporates  the  Cowper  and  Symonds  formulation  within  the  yield  surface.    An 
additional cost is incurred but the improvement is results can be dramatic.
*MAT_STRAIN_RATE_DEPENDENT_PLASTICITY 
This  is  Material  Type  19.    A  strain  rate  dependent  material  can  be  defined.    For  an 
alternative,  see  Material  Type  24.    Required  is  a  curve  for  the  yield  stress  versus  the 
effective strain rate.  Optionally, Young’s modulus and the tangent modulus can also be 
defined  versus  the  effective  strain  rate.    Also,  optional  failure  of  the  material  can  be 
defined  either  by  defining  a  von  Mises  stress  at  failure  as  a  function  of  the  effective 
strain rate (valid for solids/shells/thick shells) or by defining a minimum time step size 
(only for shells). 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
VP 
F 
Default 
none 
none 
none 
none 
0.0 
6 
7 
8 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LC1 
ETAN 
LC2 
LC3 
LC4 
TDEL 
RDEF 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
VP 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
Formulation for rate effects: 
EQ.0.0: Scale yield stress (default), 
EQ.1.0: Viscoplastic formulation
LC1 
ETAN 
LC2 
LC3 
LC4 
TDEL 
*MAT_STRAIN_RATE_DEPENDENT_PLASTICITY 
DESCRIPTION
Load  curve  ID  defining  the  yield  stress  σ0  as  a  function  of  the 
effective strain rate. 
Tangent modulus, Et 
Load  curve  ID  defining  Young’s  modulus  as  a  function  of  the
effective 
(available  only  when  VP = 0;  not 
strain 
recommended). 
rate 
Load  curve  ID  defining  tangent  modulus  as  a  function  of  the
effective strain rate (optional). 
Load curve ID defining von Mises stress at failure as a function of
the effective strain rate (optional). 
Minimum time step size for automatic element deletion.  Use for
shells only. 
RDEF 
Redefinition of failure curve: 
EQ.1.0: Effective plastic strain, 
EQ.2.0: Maximum  principal  stress  and  absolute  value  of
minimum principal stress, 
EQ.3.0: Maximum principal stress (release 5 of  v.971) 
Remarks: 
In  this  model,  a  load  curve  is  used  to  describe  the  yield  strength  𝜎0  as  a  function  of 
effective strain rate 𝜀̅
̇ where 
𝜀̅
̇ = (
2⁄
′ )
′ 𝜀̇𝑖𝑗
𝜀̇𝑖𝑗
and the prime denotes the deviatoric component.  The strain rate is available for post-
processing  as  the  first  stored  history  variable.    If  the  viscoplastic  option  is  active,  the 
plastic strain rate is output; otherwise, the effective strain rate defined above is output.   
The yield stress is defined as 
𝜎𝑦 = 𝜎0(𝜀̅
̇) + 𝐸𝑝𝜀̅𝑝 
where 𝜀̅𝑝 is the effective plastic strain and 𝐸𝑝 is given in terms of Young’s modulus and 
the tangent modulus by
𝐸𝑝 =
𝐸𝐸𝑡
𝐸 − 𝐸𝑡
. 
Both Young's modulus and the tangent modulus may optionally be made functions of 
strain rate by specifying a load curve ID giving their values as a function of strain rate.  
If these load curve ID's are input as 0, then the constant values specified in the input are 
used. 
Note that all load curves used to define quantities as a function of strain rate must have 
the same number of points at the same strain rate values.  This requirement is used to 
allow  vectorized  interpolation  to  enhance  the  execution  speed  of  this  constitutive 
model. 
This  model  also  contains  a  simple  mechanism  for  modeling  material  failure.    This 
option is activated by specifying a load curve ID defining the effective stress at failure 
as  a  function  of  strain  rate.    For  solid  elements,  once  the  effective  stress  exceeds  the 
failure  stress  the  element  is  deemed  to  have  failed  and  is  removed  from  the  solution.  
For  shell  elements  the  entire  shell  element  is  deemed  to  have  failed  if  all  integration 
points  through  the  thickness  have  an  effective  stress  that  exceeds  the  failure  stress.  
After failure the shell element is removed from the solution. 
In  addition  to  the  above  failure  criterion,  this  material  model  also  supports  a  shell 
element deletion criterion based on the maximum stable time step size for the element, 
Δ𝑡max.  Generally, Δ𝑡max goes down as the element becomes more distorted.  To assure 
stability of time integration, the global LS-DYNA time step is the minimum of the Δ𝑡max 
values  calculated  for  all  elements  in  the  model.    Using this  option allows  the  selective 
deletion  of  elements  whose  time  step  Δ𝑡max  has  fallen  below  the  specified  minimum 
time step, Δ𝑡crit.  Elements which are severely distorted often indicate that material has 
failed and supports little load, but these same elements may have very small time steps 
and therefore control the cost of the analysis.  This option allows these highly distorted 
elements to be deleted from the calculation, and, therefore, the analysis can proceed at a 
larger time step, and, thus, at a reduced cost.  Deleted elements do not carry any load, 
and are deleted from all applicable slide surface definitions.  Clearly, this option must 
be judiciously used to obtain accurate results at a minimum cost. 
A  fully  viscoplastic  formulation  is  optional  which  incorporates  the  rate  formulation 
within the yield surface.  An additional cost is incurred but the improvement is results 
can be dramatic.
*MAT_RIGID 
This  is  Material  20.    Parts  made  from  this  material  are  considered to  belong  to  a  rigid 
body (for each part ID).  Also, the coupling of a rigid body with MADYMO and CAL3D 
can  be  defined  via  this  material.    Alternatively,  a  VDA  surface  can  be  attached  as 
surface to model the geometry, e.g., for the tooling in metalforming applications.  Also, 
global and local constraints on the mass center can be optionally defined.  Optionally, a 
local consideration for output and user-defined airbag sensors can be chosen. 
5 
N 
F 
0 
5 
  Card 1 
1 
2 
Variable 
MID 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
Default 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
Variable 
CMO 
CON1 
CON2 
Type 
Default 
F 
0 
F 
0 
F 
0 
Optional for output (Must be included but may be left blank).  
  Card 3 
1 
2 
Variable  LCO or A1 
A2 
Type 
Default 
F 
0 
F 
0 
3 
A3 
F 
0 
4 
V1 
F 
0 
5 
V2 
F 
0 
7 
M 
F 
0 
7 
8 
ALIAS or
RE 
C/F 
blank 
none 
8 
7 
8 
6 
COUPLE 
F 
0 
6 
6 
V3 
F
MID 
RO 
E 
PR 
N 
*MAT_020 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s  modulus.    Reasonable  values  have  to  be  chosen  for
contact analysis (choice of penalty), see Remarks below. 
Poisson’s ratio.  Reasonable values have to be chosen for contact
analysis (choice of penalty), see Remarks below. 
MADYMO3D 5.4 coupling flag, n: 
EQ.0: use normal LS-DYNA rigid body updates, 
GT.0:  the  rigid  body  is  coupled  to  MADYMO  5.4  ellipsoid
number n 
LT.0:  the rigid body is coupled to MADYMO 5.4 plane number
|n|. 
COUPLE 
Coupling option if applicable: 
EQ.-1:  attach  VDA  surface  in  ALIAS  (defined  in  the  eighth
field)  and  automatically  generate  a  mesh  for  viewing
the surface in LS-PREPOST. 
MADYMO 5.4 / CAL3D coupling option: 
EQ.0:  the  undeformed  geometry 
to  LS-DYNA 
corresponds  to  the  local  system  for  MADYMO  5.4  /
CAL3D.  The finite element mesh is input, 
input 
EQ.1:  the  undeformed  geometry 
to  LS-DYNA 
corresponds  to  the  global  system  for  MADYMO  5.4  /
CAL3D, 
input 
EQ.2:  generate a mesh for the ellipsoids and planes internally
in LS-DYNA. 
M 
MADYMO3D 5.4 coupling flag, m: 
EQ.0:  use normal LS-DYNA rigid body updates, 
EQ.m:  this  rigid  body  corresponds  to  MADYMO  rigid  body
number  m.    Rigid  body  updates  are  performed  by
MADYMO. 
ALIAS 
VDA surface alias name, see Appendix L.
RE 
CMO 
DESCRIPTION
MADYMO 6.0.1 External Reference Number 
Center of mass constraint option, CMO: 
EQ.+1.0: constraints applied in global directions, 
EQ.0.0:  no constraints, 
*MAT_RIGID 
EQ.-1.0:  constraints 
constraint). 
applied 
in 
local  directions 
(SPC 
CON1 
First constraint parameter: 
If CMO = +1.0, then specify global translational constraint: 
EQ.0: no constraints, 
EQ.1: constrained x displacement, 
EQ.2: constrained y displacement, 
EQ.3: constrained z displacement, 
EQ.4: constrained x and y displacements, 
EQ.5: constrained y and z displacements, 
EQ.6: constrained z and x displacements, 
EQ.7: constrained x, y, and z displacements. 
If CM0 = -1.0, then specify local coordinate system ID.  
See  *DEFINE_COORDINATE_OPTION:    This  coordinate 
system is fixed in time. 
CON2 
Second constraint parameter: 
If CMO = +1.0, then specify global rotational constraint: 
EQ.0: no constraints, 
EQ.1: constrained x rotation, 
EQ.2: constrained y rotation, 
EQ.3: constrained z rotation, 
EQ.4: constrained x and y rotations, 
EQ.5: constrained y and z rotations, 
EQ.6: constrained z and x rotations, 
EQ.7: constrained x, y, and z rotations.
VARIABLE   
DESCRIPTION
If CM0 = -1.0, then specify local (SPC) constraint: 
EQ.000000:  no constraint, 
EQ.100000:  constrained x translation, 
EQ.010000:  constrained y translation, 
EQ.001000:  constrained z translation, 
EQ.000100:  constrained x rotation, 
EQ.000010:  constrained y rotation, 
EQ.000001:  constrained z rotation. 
Any  combination  of  local  constraints  can  be  achieved  by  adding
the number 1 into the corresponding column. 
LCO 
Local coordinate system number for output. 
A1 - V3 
Alternative method for specifying local system below: 
Define two vectors a and v, fixed in the rigid body which are 
used  for  output  and  the  user  defined  airbag  sensor  subrou-
tines.  The output parameters are in the directions a, b, and c
where the latter are given by the cross products c = a × v and 
b = c × a.  This input is optional. 
Remarks: 
The  rigid  material  type  20  provides  a  convenient  way  of  turning  one  or  more  parts 
comprised  of  beams,  shells,  or  solid  elements  into  a  rigid  body.    Approximating  a 
deformable  body  as  rigid  is  a  preferred  modeling  technique  in  many  real  world 
applications.    For  example,  in  sheet  metal  forming  problems  the  tooling  can  properly 
and accurately be treated as rigid.  In the design of restraint systems the occupant can, 
for  the  purposes  of  early  design  studies,  also  be  treated  as  rigid.    Elements  which  are 
rigid  are  bypassed  in  the  element  processing  and  no  storage  is  allocated  for  storing 
history variables; consequently, the rigid material type is very cost efficient. 
Two  unique  rigid  part  ID's  may  not  share  common  nodes  unless  they  are  merged 
together using the rigid body merge option.  A rigid body may be made up of disjoint 
finite  element  meshes,  however.    LS-DYNA  assumes  this  is  the  case  since  this  is  a 
common practice in setting up tooling meshes in forming problems. 
All elements which reference a given part ID corresponding to the rigid material should 
be  contiguous,  but  this  is  not  a  requirement.    If  two  disjoint  groups  of  elements  on 
opposite sides of a model are modeled as rigid, separate part ID's should be created for
each  of  the  contiguous  element  groups  if  each  group  is  to  move  independently.    This 
requirement arises from the fact that LS-DYNA internally computes the six rigid body 
degrees-of-freedom for each rigid body (rigid material or set of merged materials), and 
if disjoint groups of rigid elements use the same part ID, the disjoint groups will move 
together as one rigid body. 
Inertial properties for rigid materials may be defined in either of two ways.  By default, 
the  inertial  properties  are  calculated  from  the  geometry  of  the  constituent  elements  of 
the  rigid  material  and  the  density  specified  for  the  part  ID.    Alternatively,  the  inertial 
properties  and  initial  velocities  for  a  rigid  body  may  be  directly  defined,  and  this 
overrides  data  calculated  from  the  material  property  definition  and  nodal  initial 
velocity definitions. 
Young's  modulus,  E,  and  Poisson's  ratio,  υ  are  used  for  determining  sliding  interface 
parameters if the rigid body interacts in a contact definition.  Realistic values for these 
constants  should  be  defined  since  unrealistic  values  may  contribute  to  numerical 
problem in contact. 
Constraint directions for rigid materials (CMO equal to +1 or -1) are fixed, that is, not 
updated,  with  time.    To  impose  a  constraint  on  a  rigid  body  such  that  the  constraint 
direction  is  updated  as  the  rigid  body  rotates,  use  *BOUNDARY_PRESCRIBED_MO-
TION_RIGID_LOCAL. 
It  is  strongly  advised  that  nodal  constraints,  e.g.,  by  *BOUNDARY_SPC_OPTION,  not 
be  applied  to  nodes  of  a  rigid  body  as  doing  so  may  compromise  the  intended 
constraints  in  the  case  of  an  explicit  simulation.    Such  SPCs  will  be  skipped  in  an 
implicit simulation and a warning issued.   
If  the  intended  constraints  are  not  with  respect  to  the  calculated  center-of-mass  of  the 
rigid body, *CONSTRAINED_JOINT_OPTION may often be used to obtain the desired 
effect.    This  approach  typically  entails  defining  a  second  rigid  body  which  is  fully 
constrained and then defining a joint between the two rigid bodies.  Another alternative 
for defining rigid body constraints that are not with respect to the calculated center-of-
mass  of  the  rigid  body  is  to  manually  specify  the  initial  center-of-mass  location  using 
*PART_INERTIA.  When using *PART_INERTIA, a full set of mass properties must be 
specified and the user must understand that the dynamic behavior of the rigid body is 
affected by its mass properties. 
For coupling with MADYMO 5.4.1, only basic coupling is available. 
The  coupling  flags  (N  and  M)  must  match  with  SYSTEM  and  ELLIP-
SOID/PLANE in the MADYMO input file and the coupling option (COUPLE) 
must be defined.
For coupling with MADYMO 6.0.1, both basic and extended coupling are available: 
1.  Basic  Coupling:    The  external  reference  number  (RE)  must  match  with  the 
external  reference  number  in  the  MADYMO  XML  input  file.    The  coupling 
option (COUPLE) must be defined. 
2.  Extended  Coupling:    Under  this  option  MADYMO  will  handle  the  contact 
between the MADYMO and LS-DYNA models.  The external reference number 
(RE) and the coupling option (COUPLE) are not needed.  All coupling surfaces 
that interface with the MADYMO models need to be defined in *CONTACT_-
COUPLING.
*MAT_ORTHOTROPIC_THERMAL_{OPTION} 
This  is  Material  Type  21.    A  linearly  elastic,  orthotropic  material  with  orthotropic 
thermal expansion. 
Available options include: 
<BLANK> 
FAILURE 
CURING 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
EA 
F 
3 
Variable 
GAB 
GBC 
GCA 
Type 
F 
F 
F 
  Card 3 
Variable 
1 
XP 
Type 
F 
  Card 4 
Variable 
1 
V1 
Type 
F 
2 
YP 
F 
2 
V2 
F 
3 
ZP 
F 
3 
V3 
F 
4 
EB 
F 
4 
AA 
F 
4 
A1 
F 
4 
D1 
F 
5 
EC 
F 
5 
AB 
F 
5 
A2 
F 
5 
D2 
F 
6 
7 
8 
PRBA 
PRCA 
PRCB 
F 
6 
AC 
F 
6 
A3 
F 
6 
D3 
F 
F 
7 
F 
8 
AOPT 
MACF 
F 
7 
I 
8 
7 
8 
BETA 
REF
Required for failure. 
  Card 5 
Variable 
1 
A1 
2 
A11 
Type 
F 
F 
3 
A2 
F 
Additional card 5 required for curing. 
  Card 5 
Variable 
1 
K1 
Type 
F 
2 
K2 
F 
3 
C1 
F 
Additional card 6 required for curing. 
4 
A5 
F 
4 
C2 
F 
5 
A55 
F 
5 
M 
F 
6 
A4 
F 
6 
N 
F 
7 
NIP 
F 
7 
R 
F 
8 
8 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCCHA 
LCCHB 
LCCHC 
LCAA 
LCAB 
LCAC 
Type 
I 
I 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
MID 
RO 
EA 
EB 
EC 
PRBA 
PRCA 
PRCB 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
𝐸𝑎, Young’s modulus in 𝑎-direction. 
𝐸𝑏, Young’s modulus in 𝑏-direction. 
𝐸𝑐, Young’s modulus in 𝑐-direction. 
𝜈𝑏𝑎, Poisson’s ratio, 𝑏𝑎. 
𝜈𝑐𝑎, Poisson’s ratio, 𝑐𝑎. 
𝜈𝑐𝑏, Poisson’s ratio, 𝑐𝑏
*MAT_ORTHOTROPIC_THERMAL 
DESCRIPTION
GAB 
GBC 
GCA 
AA 
AB 
AC 
AOPT 
𝐺𝑎𝑏, Shear modulus, 𝑎𝑏. 
𝐺𝑏𝑐, Shear modulus, 𝑏𝑐. 
𝐺𝑐𝑎, Shear modulus, 𝑐𝑎. 
𝛼𝑎, coefficient of thermal expansion in the 𝑎-direction. 
𝛼𝑏, coefficient of thermal expansion in the 𝑏-direction. 
𝛼𝑐, coefficient of thermal expansion in the 𝑐-direction. 
Material axes option : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES, and then, for shells only, rotated about
the shell element normal by an angle BETA. 
EQ.1.0: locally orthotropic with material axes determined by a
point  in  space  and  the  global  location  of  the  element
center;  this  is  the  a-direction.    This  option  is  for  solid 
elements only. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by 
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the
element normal. 
EQ.4.0: locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector  𝐯,  and 
an originating point, 𝐩, which define the centerline ax-
is.  This option is for solid elements only. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later.
VARIABLE   
DESCRIPTION
MACF 
Material axes change flag for brick elements: 
EQ.1: No change, default, 
EQ.2: switch material axes a and b, 
EQ.3: switch material axes a and c, 
EQ.4: switch material axes b and c. 
XP, YP, ZP 
Coordinates of point 𝐩 for AOPT = 1 and 4. 
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3 and 4. 
D1, D2, D3 
Components of vector 𝐝 for AOPT = 2. 
BETA 
REF 
Material  angle  in  degrees  for  AOPT = 1  (shells  only)  and 
AOPT = 3,  may  be  overridden  on  the  element  card,  see  *ELE-
MENT_SHELL_BETA or *ELEMENT_SOLID_ORTHO. 
Use  reference  geometry  to  initialize  the  stress  tensor.    The
reference geometry is defined by the keyword:*INITIAL_FOAM_-
REFERENCE_GEOMETRY . 
EQ.0.0: off, 
EQ.1.0: on. 
A1, A11, A2 
A5, A55, A4 
Coefficients for the matrix dominated failure criterion. 
Coefficients for the fiber dominated failure criterion. 
K1 
K2 
C1 
C2 
M 
N 
R 
Parameter 𝑘1 for Kamal model.  For details see remark below. 
Parameter 𝑘2 for Kamal model. 
Parameter 𝑐1 for Kamal model. 
Parameter 𝑐2 for Kamal model. 
Exponent 𝑚 for Kamal model. 
Exponent 𝑛 for Kamal model. 
Gas constant for Kamal model.
LCCHA 
LCCHB 
LCCHC 
LCAA 
*MAT_ORTHOTROPIC_THERMAL 
DESCRIPTION
Load  curve  for  𝛾𝑎,  coefficient  of  chemical  shrinkage  in  the  𝑎-
direction.  Input 𝛾𝑎 as function of state of cure 𝛽. 
Load  curve  for  𝛾𝑏,  coefficient  of  chemical  shrinkage  in  the  𝑏-
direction.  Input 𝛾𝑏 as function of state of cure 𝛽. 
Load  curve  for  𝛾𝑐,  coefficient  of  chemical  shrinkage  in  the  𝑐-
direction.  Input 𝛾𝑐 as function of state of cure 𝛽. 
Load  curve  or  table  ID  for  𝛼𝑎.    If  defined  parameter  AA  is 
ignored.  
IF LCID 
Input 𝛼𝑎 versus temperature. 
IF TABID: 
Input  𝛼𝑎  as  functions  of  state  of  cure  (table  values)  and 
temperatures  
Load  curve  ID  for  𝛼𝑏.    If  defined  parameter  AB  is  ignored.    See 
LCAA for further details. 
Load  curve  ID  for  𝛼𝑐.    If  defined  parameter  AC  is  ignored.    See 
LCAA for further details. 
LCAB 
LCAC 
Remarks: 
In the implementation for three-dimensional continua a total Lagrangian formulation is 
used.  In this approach the material law that relates second Piola-Kirchhoff stress  𝐒 to 
the Green-St.  Venant strain 𝐄 is 
where 𝐓 is the transformation matrix [Cook 1974]. 
𝐒 = 𝐂 ⋅ 𝐄 = 𝐓T𝐂𝑙𝐓 ⋅ 𝐄 
𝐓 =  
𝑙1
𝑙2
𝑙3
2𝑙1𝑙2
2𝑙2𝑙3
2𝑙3𝑙1
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
𝑚1
𝑚2
𝑚3
2𝑚1𝑚2
2𝑚2𝑚3
2𝑚3𝑚1
𝑛1
𝑛2
𝑚3
2𝑛1𝑛2
2𝑛2𝑛3
2𝑛3𝑛1
𝑙1𝑚1
𝑙2𝑚2
𝑙3𝑚3
(𝑙1𝑚2 + 𝑙2𝑚1)
(𝑙2𝑚3 + 𝑙3𝑚2)
(𝑙3𝑚1 + 𝑙1𝑚3)
𝑚1𝑛1
𝑚2𝑛2
𝑚3𝑛3
(𝑚1𝑛2 + 𝑚2𝑛1)
(𝑚2𝑛3 + 𝑚3𝑛2)
(𝑚3𝑛1 + 𝑚1𝑛3)
𝑛1𝑙1
⎤
⎥
𝑛2𝑙2
⎥
⎥
𝑛3𝑙3
⎥
⎥
(𝑛1𝑙2 + 𝑛2𝑙1)
⎥
(𝑛2𝑙3 + 𝑛3𝑙2)
⎥
(𝑛3𝑙1 + 𝑛1𝑙3)⎦
𝑙𝑖, 𝑚𝑖, 𝑛𝑖 are the direction cosines 
′ = 𝑙𝑖𝑥1 + 𝑚𝑖𝑥2 + 𝑛𝑖𝑥3 for  𝑖 = 1, 2, 3 
𝑥𝑖
′ denotes the material axes.  The constitutive matrix 𝐂𝑙 is defined in terms of the 
and 𝑥𝑖
material axes as 
−1 =  
𝐂𝑙
𝐸11
𝜐12
𝐸11
𝜐13
𝐸11
−
−
−
𝜐21
𝐸22
𝐸22
𝜐23
𝐸22
−
−
−
𝜐31
𝐸33
𝜐32
𝐸33
𝐸33
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
𝐺12
𝐺23
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
𝐺31 ⎦
where the subscripts denote the material axes, i.e., 
′ 
′      and      𝐸𝑖𝑖 = 𝐸𝑥𝑖
𝜐𝑖𝑗 = 𝜐𝑥𝑖
′𝑥𝑗
Since 𝐂𝑙 is symmetric 
𝜐12
𝐸11
=
𝜐21
𝐸22
, … 
The vector of Green-St.  Venant strain components is 
𝐄T = [𝐸11, 𝐸22, 𝐸33, 𝐸12, 𝐸23, 𝐸31] 
which include the local thermal strains which are integrated in time: 
𝑛+1 = 𝜀𝑎𝑎
𝜀𝑎𝑎
𝑛+1 = 𝜀𝑏𝑏
𝜀𝑏𝑏
𝑛+1 = 𝜀𝑐𝑐
𝜀𝑐𝑐
𝑛 + 𝛼𝑎(𝑇𝑛+1 − 𝑇𝑛) 
𝑛 + 𝛼𝑏(𝑇𝑛+1 − 𝑇𝑛) 
𝑛 + 𝛼𝑐(𝑇𝑛+1 − 𝑇𝑛) 
where 𝑇 is temperature.  After computing 𝑆𝑖𝑗 we then obtain the Cauchy stress: 
𝜎𝑖𝑗 =
𝜌0
∂𝑥𝑖
∂𝑋𝑘
∂𝑥𝑗
∂𝑋𝑙
𝑆𝑘𝑙 
This model will predict realistic behavior for finite displacement and rotations as long 
as the strains are small. 
In  the  implementation  for  shell  elements,  the  stresses  are  integrated  in  time  and  are 
updated in the corotational coordinate system.  In this procedure the local material axes 
are  assumed  to  remain  orthogonal  in  the  deformed  configuration.   This  assumption  is 
valid if the strains remain small.
The  failure  models  were  derived  by  William  Feng.    The  first  one  defines  the  matrix 
dominated failure mode, 
𝐹𝑚 = 𝐴1(𝐼1 − 3) + 𝐴11(𝐼1 − 3)2 + 𝐴2(𝐼2 − 3) − 1 
and the second defines the fiber dominated failure mode, 
𝐹𝑓 = 𝐴5(𝐼5 − 1) + 𝐴55(𝐼5 − 1)2 + 𝐴4(𝐼4 − 1) − 1. 
When either is greater than zero, the integration point fails, and the element is deleted 
after NIP integration points fail. 
The coefficients 𝐴𝑖 are defined in the input and the invariants 𝐼𝑖 are the strain invariants 
𝐼1 = ∑ 𝐶𝛼𝛼
𝛼=1,3
𝐼2 =
[𝐼1
2 − ∑ 𝐶𝛼𝛽
𝛼,𝛽=1,3
] 
𝐼3 = det(𝐂) 
𝐼4 = ∑ 𝑉𝛼
𝛼,𝛽,𝛾=1,3
𝐶𝛼𝛾𝐶𝛾𝛽𝑉𝛽 
𝐼5 = ∑ 𝑉𝛼
𝛼,𝛽=1,3
𝐶𝛼𝛽𝑉𝛽 
and 𝐂 is the Cauchy strain tensor and 𝐕 is the fiber direction in the undeformed state.  
By convention in this material model, the fiber direction is aligned with the 𝑎 direction 
of the local orthotropic coordinate system.  
The  curing  option  implies  that  orthotropic  chemical  shrinkage  is  to  be  considered, 
resulting  from  a  curing  process  in  the  material.    The  state  of  cure  𝛽  is  an  internal 
material variable that follows the Kamal model 
= (𝐾1 + 𝐾2𝛽𝑚)(1 − 𝛽)𝑛    with      𝐾1 = 𝑘1𝑒
−
𝑐1
𝑅𝑇,   𝐾2 = 𝑘2𝑒
−
𝑐2
𝑅𝑇 
𝑑𝛽
𝑑𝑡
and chemical strains are introduced: 
𝑛+1 = 𝜀𝑎𝑎
𝜀𝑎𝑎
𝑛+1 = 𝜀𝑏𝑏
𝜀𝑏𝑏
𝑛+1 = 𝜀𝑐𝑐
𝜀𝑐𝑐
𝑛 + 𝛾𝑎(𝛽𝑛+1 − 𝛽𝑛) 
𝑛 + 𝛾𝑏(𝛽𝑛+1 − 𝛽𝑛) 
𝑛 + 𝛾𝑐(𝛽𝑛+1 − 𝛽𝑛) 
The coefficients 𝛾𝑎, 𝛾𝑏, 𝛾𝑐 can be defined as functions of the state of cure 𝛽.  Furthermore, 
the  coefficients  of  thermal  expansion  𝛼𝑎, 𝛼𝑏, 𝛼𝑐can  also  be  defined  as  functions  of  the 
state of cure 𝛽 and the temperature 𝑇, if the curing option is used.
*MAT_022 
This  is  Material  Type  22.    An  orthotropic  material  with  optional  brittle  failure  for 
composites  can  be  defined  following  the  suggestion  of  [Chang  and  Chang  1987a, 
1987b].  Three failure criteria are possible, see the LS-DYNA Theory Manual.  By using 
the  user  defined  integration  rule,  see  *INTEGRATION_SHELL,  the  constitutive 
constants can vary through the shell thickness. 
For  all  shells,  except  the  DKT  formulation,  laminated  shell  theory  can  be  activated  to 
properly  model  the  transverse  shear  deformation.    Lamination  theory  is  applied  to 
correct  for  the  assumption  of  a  uniform  constant  shear  strain through  the  thickness  of 
the  shell.    For  sandwich  shells  where  the  outer  layers  are  much  stiffer  than  the  inner 
layers, the response will tend to be too stiff unless lamination theory is used.  To turn on 
lamination theory see *CONTROL_SHELL. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
EA 
F 
4 
EB 
F 
5 
EC 
F 
6 
7 
8 
PRBA 
PRCA 
PRCB 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
GAB 
GBC 
GCA 
KFAIL 
AOPT 
MACF 
ATRACK 
Type 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
0.0 
0.0 
I 
0 
I
Variable 
1 
XP 
Type 
F 
*MAT_COMPOSITE_DAMAGE 
2 
YP 
F 
3 
ZP 
F 
4 
A1 
F 
5 
A2 
F 
6 
A3 
F 
7 
8 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 4 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
7 
8 
BETA 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 5 
Variable 
1 
SC 
Type 
F 
2 
XT 
F 
3 
YT 
F 
4 
YC 
F 
5 
ALPH 
F 
6 
SN 
F 
7 
8 
SYZ 
SZX 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
MID 
RO 
EA 
EB 
EC 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
𝐸𝑎, Young’s modulus in 𝑎-direction. 
𝐸𝑏, Young’s modulus in 𝑏-direction. 
𝐸𝑐, Young’s modulus in 𝑐-direction. 
PRBA 
𝜈𝑏𝑎, Poisson ratio, 𝑏𝑎.
VARIABLE   
DESCRIPTION
PRCA 
PRCB 
GAB 
GBC 
GCA 
KFAIL 
AOPT 
𝜈𝑐𝑎, Poisson ratio, 𝑐𝑎. 
𝜈𝑐𝑏, Poisson ratio, 𝑐𝑏. 
𝐺𝑎𝑏, Shear modulus, 𝑎𝑏. 
𝐺𝑏𝑐, Shear modulus, 𝑏𝑐. 
𝐺𝑐𝑎, Shear modulus, 𝑐𝑎. 
Bulk  modulus  of  failed  material.    Necessary  for  compressive 
failure. 
Material axes option : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES, and then, for shells only, rotated about 
the shell element normal by an angle BETA.  
EQ.1.0: locally orthotropic with material axes determined by a
point  in  space  and  the  global  location  of  the  element
center;  this  is  the  𝑎-direction.    This  option  is  for  solid 
elements only. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element 
defined  by  the  cross  product  of  the  vector  v  with  the
element normal. 
EQ.4.0: locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector  𝐯,  and 
an originating point, 𝐩, which define the centerline ax-
is.  This option is for solid elements only. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later.
*MAT_COMPOSITE_DAMAGE 
DESCRIPTION
MACF 
Material axes change flag for brick elements: 
EQ.1: No change, default, 
EQ.2: switch material axes 𝑎 and 𝑏, 
EQ.3: switch material axes 𝑎 and 𝑐, 
EQ.4: switch material axes 𝑏 and 𝑐. 
ATRACK 
Material a-axis tracking flag (shell elements only) 
EQ.0:  a-axis rotates with element (default) 
EQ.1:  a-axis also tracks deformation 
XP, YP, ZP 
Coordinates of point 𝐩 for AOPT = 1 and 4. 
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3 and 4. 
D1, D2, D3 
Components of vector 𝐝 for AOPT = 2. 
Material  angle  in  degrees  for  AOPT = 0  (shells  only)  and 
AOPT = 3,  may  be  overridden  on  the  element  card,  see  *ELE-
MENT_SHELL_BETA or *ELEMENT_SOLID_ORTHO. 
Shear strength, ab plane, see the LS-DYNA Theory Manual. 
Longitudinal  tensile  strength,  𝑎-axis,  see  the  LS-DYNA  Theory 
Manual. 
Transverse tensile strength, 𝑏-axis. 
Transverse compressive strength, 𝑏-axis (positive value). 
Shear  stress  parameter  for  the  nonlinear  term,  see  the  LS-DYNA 
Theory Manual.  Suggested range 0 – 0.5. 
Normal tensile strength (solid elements only) 
Transverse shear strength (solid elements only) 
Transverse shear strength (solid elements only) 
BETA 
SC 
XT 
YT 
YC 
ALPH 
SN 
SYZ 
SZX 
Remarks: 
1.  History  Data.    The  number  of  additional  integration  point  variables  for  shells 
written to the d3plot database is specified using the *DATABASE_EXTENT_BI-
NARY  keyword  on  the  NEIPS  field.    These  additional  history  variables  are 
enumerated below: 
History Variable3 
Description 
Value 
ef(𝑖)  
tensile fiber mode 
LS-PrePost 
history variable
See 
below 
table 
cm(𝑖)  
ed(𝑖)  
tensile matrix mode 
compressive 
mode 
matrix 
1 - elastic 
0 - failed 
1 
2 
The  following  components  are  stored  as  element  component  7  instead  of  the 
effective plastic strain.  Note that ef(𝑖) for 𝑖 = 1,2,3 is not retrievable. 
Description 
Integration point 
nip
nip
∑ ef(𝑖)
𝑖=1
nip
nip
∑ cm(𝑖)
𝑖=1
nip
nip
∑ ed(𝑖)
𝑖=1
ef(𝑖) for 𝑖 > 3 
1 
2 
3 
𝑖 
2.  The ATRACK Field.  The initial material directions are set using AOPT and the 
related  data.   By  default,  the  material  directions  in  shell  elements  are  updated 
each cycle based on the rotation of the 1-2 edge, or else the rotation of all edges 
if  the  invariant  node  numbering  option  is  set  on  *CONTROL_ACCURACY.  
When  ATRACK=1,  an  optional  scheme  is  used  in  which  the  𝑎-direction  of  the 
material tracks element deformation as well as rotation. 
At  the  start  of  the  calculation,  a  line  is  passed  through  each  element  center  in 
the  direction  of  the  material  a-axis.    This  line  will  intersect  the  edges  of  the 
element  at  two  points.    The  referential  coordinates  of  these  two  points  are 
stored,  and  then  used  throughout  the  calculation  to  locate  these  points  in  the 
deformed geometry.  The material 𝑎-axis is assumed to be in the direction of the 
line  that  passes  through  both  points.    If  ATRACK = 0,  the  layers  of  a  layered 
3 (cid:1861)	ranges over the shell integration points.
composite will always rotate together.  However, if ATRACK = 1, the layers can 
rotate  independently  which  may  be  more  accurate,  particularly  for  shear  de-
formation.  This option is available only for shell elements.
*MAT_TEMPERATURE_DEPENDENT_ORTHOTROPIC 
This  is  Material  Type  23.    An  orthotropic  elastic  material  with  arbitrary  temperature 
dependency can be defined. 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
4 
5 
6 
7 
8 
AOPT 
REF 
MACF 
Type 
A8 
F 
F 
F 
I 
  Card 2 
Variable 
1 
XP 
Type 
F 
  Card 3 
Variable 
1 
V1 
Type 
F 
2 
YP 
F 
2 
V2 
F 
3 
ZP 
F 
3 
V3 
F 
4 
A1 
F 
4 
D1 
F 
5 
A2 
F 
5 
D2 
F 
6 
A3 
F 
6 
D3 
F 
7 
8 
7 
8 
BETA 
F 
Temperature  Card  Pairs.    Define  one  set  of  constants  on  two  cards  using  formats  4 
and 5 for each temperature point.  Up to 48 points (96 cards) can be defined.  The next 
“*” card terminates the input. 
First Temperature Card. 
  Card 4 
1 
Variable 
EAi 
2 
EBi 
3 
4 
5 
6 
7 
8 
ECi 
PRBAi 
PRCAi 
PRCBi 
Type 
F 
F 
F 
F 
F
Second Temperature Card 
  Card 5 
1 
Variable 
AAi 
2 
ABi 
3 
4 
5 
6 
ACi 
GABi 
GBCi 
GCAi 
Type 
F 
F 
F 
F 
F 
F 
8 
7 
Ti 
F 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density. 
AOPT 
Material  axes  option  : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by 
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES, and then, for shells only, rotated about
the shell element normal by an angle BETA. 
EQ.1.0: locally orthotropic with material axes determined by a
point  in  space  and  the  global  location  of  the  element
center;  this  is  the  𝑎-direction.    This  option  is  for  solid 
elements only. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  𝐯  with  the 
element normal. 
EQ.4.0: locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector  𝐯,  and 
an originating point, 𝐩, which define the centerline ax-
is.  This option is for solid elements only. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971
VARIABLE   
DESCRIPTION
and later. 
REF 
Use  reference  geometry  to  initialize  the  stress  tensor.    The
reference geometry is defined by the keyword:*INITIAL_FOAM_-
REFERENCE_GEOMETRY . 
EQ.0.0: off, 
EQ.1.0: on. 
MACF 
Material axes change flag for brick elements: 
EQ.1: No change, default, 
EQ.2: switch material axes 𝑎 and 𝑏, 
EQ.3: switch material axes 𝑎 and 𝑐, 
EQ.4: switch material axes 𝑏 and 𝑐. 
XP, YP, ZP 
Coordinates of point 𝐩 for AOPT = 1 and 4. 
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3 and 4. 
D1, D2, D3 
Components of vector 𝐝 for AOPT = 2. 
BETA 
EAi 
EBi 
ECi 
PRBAi 
PRCAi 
PRCBi 
AAi 
ABi 
Material  angle  in  degrees  for  AOPT = 0  (shells  only)  and 
AOPT = 3,  may  be  overridden  on  the  element  card,  see  *ELE-
MENT_SHELL_BETA or *ELEMENT_SOLID_ORTHO. 
𝐸𝑎, Young’s modulus in 𝑎-direction at temperature Ti. 
𝐸𝑏, Young’s modulus in 𝑏-direction at temperature Ti. 
𝐸𝑐, Young’s modulus in 𝑐-direction at temperature Ti. 
𝜈𝑏𝑎, Poisson’s ratio 𝑏𝑎 at temperature Ti. 
𝜈𝑐𝑎, Poisson’s ratio 𝑐𝑎 at temperature Ti. 
𝜈𝑐𝑏, Poisson’s ratio 𝑐𝑏 at temperature Ti. 
𝛼𝑎, coefficient of thermal expansion in  𝑎-direction at temperature 
Ti. 
𝛼𝐵  coefficient  of  thermal  expansion  in  𝑏-direction  at  temperature 
Ti.
𝛼𝑐,  coefficient  of  thermal  expansion  in  𝑐-direction  at  temperature 
Ti. 
𝐺𝑎𝑏, Shear modulus 𝑎𝑏 at temperature Ti. 
𝐺𝑏𝑐, Shear modulus 𝑏𝑐 at temperature Ti. 
𝐺𝑐𝑎, Shear modulus 𝑐𝑎 at temperature Ti. 
ith temperature 
*MAT_023 
  VARIABLE   
ACi 
GABi 
GBCi 
GCAi 
Ti 
Remarks: 
In the implementation for three-dimensional continua a total Lagrangian formulation is 
used.  In this approach the material law that relates second Piola-Kirchhoff stress  𝐒 to 
the Green-St.  Venant strain 𝐄 is 
where 𝐓 is the transformation matrix [Cook 1974]. 
𝐒 = 𝐂 ⋅ 𝐄 = 𝐓T𝐂𝒍𝐓 ⋅ 𝐄 
𝐓 =  
𝑙1
𝑙2
𝑙3
2𝑙1𝑙2
2𝑙2𝑙3
2𝑙3𝑙1
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
𝑚1
𝑚2
𝑚3
2𝑚1𝑚2
2𝑚2𝑚3
2𝑚3𝑚1
𝑛1
𝑛2
𝑚3
2𝑛1𝑛2
2𝑛2𝑛3
2𝑛3𝑛1
𝑙1𝑚1
𝑙2𝑚2
𝑙3𝑚3
(𝑙1𝑚2 + 𝑙2𝑚1)
(𝑙2𝑚3 + 𝑙3𝑚2)
(𝑙3𝑚1 + 𝑙1𝑚3)
𝑚1𝑛1
𝑚2𝑛2
𝑚3𝑛3
(𝑚1𝑛2 + 𝑚2𝑛1)
(𝑚2𝑛3 + 𝑚3𝑛2)
(𝑚3𝑛1 + 𝑚1𝑛3)
𝑛1𝑙1
⎤
⎥
𝑛2𝑙2
⎥
⎥
𝑛3𝑙3
⎥
⎥
(𝑛1𝑙2 + 𝑛2𝑙1)
⎥
(𝑛2𝑙3 + 𝑛3𝑙2)
⎥
(𝑛3𝑙1 + 𝑛1𝑙3)⎦
𝑙𝑖, 𝑚𝑖, 𝑛𝑖 are the direction cosines 
′ = 𝑙𝑖𝑥1 + 𝑚𝑖𝑥2 + 𝑛𝑖𝑥3 for  𝑖 = 1, 2, 3 
𝑥𝑖
′ denotes the material axes.  The temperature dependent constitutive matrix 𝐂𝑙 is 
and 𝑥𝑖
defined in terms of the material axes as
𝐸11(𝑇)
𝜐12(𝑇)
𝐸11(𝑇)
𝜐13(𝑇)
𝐸11(𝑇)
−
−
−
𝜐21(𝑇)
𝐸22(𝑇)
𝐸22(𝑇)
𝜐23(𝑇)
𝐸22(𝑇)
−
−
−
𝜐31(𝑇)
𝐸33(𝑇)
𝜐32(𝑇)
𝐸33(𝑇)
𝐸33(𝑇)
−1 =  
𝐂𝑙
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
𝐺12(𝑇)
𝐺23(𝑇)
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
𝐺31(𝑇) ⎦
where the subscripts denote the material axes, i.e., 
′ 
′      and      𝐸𝑖𝑖 = 𝐸𝑥𝑖
𝜐𝑖𝑗 = 𝜐𝑥𝑖
′𝑥𝑗
Since 𝐂𝑙 is symmetric 
𝜐12
𝐸11
=
𝜐21
𝐸22
, … 
The vector of Green-St.  Venant strain components is 
𝐄T = ⌊𝐸11, 𝐸22, 𝐸33, 𝐸12, 𝐸23, 𝐸31⌋ 
which include the local thermal strains which are integrated in time: 
𝑛+1 = 𝜀𝑎𝑎
𝜀𝑎𝑎
𝑛 + 𝛼𝑎 (𝑇
𝑛+1
2) [𝑇𝑛+1 − 𝑇𝑛] 
𝑛+1 = 𝜀𝑏𝑏
𝜀𝑏𝑏
𝑛 + 𝛼𝑏 (𝑇
𝑛+1
2) [𝑇𝑛+1 − 𝑇𝑛] 
𝑛+1 = 𝜀𝑐𝑐
𝜀𝑐𝑐
𝑛 + 𝛼𝑐 (𝑇
𝑛+1
2) [𝑇𝑛+1 − 𝑇𝑛] 
where 𝑇 is temperature.  After computing 𝑆𝑖𝑗 we then obtain the Cauchy stress: 
𝜎𝑖𝑗 =
𝜌0
∂𝑥𝑖
∂𝑋𝑘
∂𝑥𝑗
∂𝑋𝑙
𝑆𝑘𝑙 
This model will predict realistic behavior for finite displacement and rotations as long 
as the strains are small. 
For  shell  elements,  the  stresses  are  integrated  in  time  and  are  updated  in  the 
corotational coordinate system.  In this procedure the local material axes are assumed to 
remain  orthogonal  in  the  deformed  configuration.    This  assumption  is  valid  if  the 
strains remain small.
*MAT_PIECEWISE_LINEAR_PLASTICITY_{OPTION} 
Available options include: 
<BLANK> 
LOG_INTERPOLATION 
STOCHASTIC 
MIDFAIL 
This  is  Material  Type  24,  which  is  an  elasto-plastic  material  with  an  arbitrary  stress 
versus  strain  curve  and  arbitrary  strain  rate  dependency  can  be  defined.    See  also 
Remark below.  Also, failure based on a plastic strain or a minimum time step size can 
be  defined.    For  another  model  with  a  more  comprehensive  failure  criteria  see  MAT_
MODIFIED_PIECEWISE_LINEAR_PLASTICITY.  If considering laminated or sandwich 
shells with non-uniform material properties (this is defined through the user specified 
integration rule), the model, MAT_LAYERED_LINEAR_PLASTICITY, is recommended.  
If solid elements are used and if the elastic strains before yielding are finite, the model, 
MAT_FINITE_ELASTIC_STRAIN_PLASTICITY,  treats  the  elastic  strains  using  a 
hyperelastic formulation.  
The  LOG_INTERPOLATION  option  interpolates  the  strain  rate  effect  in  table  LCSS 
with logarithmic interpolation. 
The STOCHASTIC option allows spatially varying yield and failure behavior.  See *DE-
FINE_STOCHASTIC_VARIATION for additional information. 
The  MIDFAIL  option  is  available  only  for  shell  elements.    When  included  on  the 
keyword  line,  this  option  causes  failure  to  be  checked  only  at  the  mid-plane  of  the 
element.    If  an  element  has  an  even  number  of  layers,  failure  is  checked  in  the  two 
layers closest to the mid-plane. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
6 
7 
8 
SIGY 
ETAN 
FAIL 
TDEL 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
0.0 
1021 
F
Card 2 
Variable 
Type 
Default 
1 
C 
F 
0 
  Card 3 
1 
2 
P 
F 
0 
2 
3 
4 
LCSS 
LCSR 
F 
0 
3 
F 
0 
4 
5 
VP 
F 
0 
5 
6 
7 
8 
6 
7 
8 
Variable 
EPS1 
EPS2 
EPS3 
EPS4 
EPS5 
EPS6 
EPS7 
EPS8 
Type 
Default 
F 
0 
  Card 4 
1 
F 
0 
2 
F 
0 
3 
F 
0 
4 
F 
0 
5 
F 
0 
6 
F 
0 
7 
F 
0 
8 
Variable 
ES1 
ES2 
ES3 
ES4 
ES5 
ES6 
ES7 
ES8 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
SIGY 
Yield stress.
Figure M24-1.  Rate effects may be accounted for by defining a table of curves.  If a
table ID is specified a curve ID is given for each strain rate, see *DEFINE_TABLE.
Intermediate  values  are  found  by  interpolating  between  curves.    Effective  plastic
strain  versus  yield  stress  is  expected.    If  the  strain  rate  values  fall  out  of  range,
extrapolation is not used; rather, either the first or last curve determines the yield
stress depending on whether the rate is low or high, respectively. 
  VARIABLE   
DESCRIPTION
ETAN 
Tangent modulus, ignored if (LCSS.GT.0) is defined. 
FAIL 
Failure flag. 
LT.0.0:  User defined failure subroutine, matusr_24 in dyn21.F, 
is called to determine failure 
EQ.0.0: Failure is not considered.  This option is recommended
if failure is not of interest since many calculations will
be saved. 
GT.0.0:  Effective  plastic  strain  to  failure.    When  the  plastic
strain  reaches  this  value,  the  element  is  deleted  from
the calculation. 
TDEL 
Minimum time step size for automatic element deletion. 
C 
Strain rate parameter, 𝐶, see formula below.
VARIABLE   
DESCRIPTION
P 
Strain rate parameter, 𝑃, see formula below. 
LCSS 
Load curve ID or Table ID. 
Load  Curve.    When  LCSS  is  a  Load  curve  ID,  it  is  taken  as
defining effective stress versus effective plastic strain.  If defined
EPS1 - EPS8 and ES1 - ES8 are ignored. 
Tabular  Data.    The  table  ID  defines  for  each  strain  rate  value  a
load  curve  ID  giving  the  stress  versus  effective  plastic  strain  for 
that rate, See Figure M24-1.  When the strain rate falls below the 
minimum value, the stress versus effective plastic strain curve for
the lowest value of strain rate is used.  Likewise, when the strain 
rate exceeds the maximum value the stress versus effective plastic
strain curve for the highest value of strain rate is used.  The strain
rate  parameters:  C  and  P,  the  curve  ID,  LCSR,  EPS1 -  EPS8,  and 
  Linear
ES1 -  ES8  are  ignored  if  a  Table  ID  is  defined. 
interpolation between the discrete strain rates is used by default;
logarithmic 
the
LOG_INTERPOLATION option is invoked. 
interpolation 
when 
used 
is 
interpolation  between  discrete  strain  rates 
Logarithmically  Defined  Tables.    An  alternative  way  to  invoke 
logarithmic 
is
described as follows.  If the first value in the table is negative, LS-
DYNA  assumes  that  all  the  table  values  represent  the  natural
logarithm  of  a  strain  rate.    Since  the  tables  are  internally 
discretized to equally space the table values, it makes good sense
from  an  accuracy  standpoint  that  the  table  values  represent  the
natural log of strain rate when the lowest strain rate and highest
strain  rate  differ  by  several  orders  of  magnitude.    There  is  some 
additional  computational  cost  associated  invoking  logarithmic
interpolation. 
Load curve ID defining strain rate scaling effect on yield stress.  If
LCSR  is  negative,  the  load  curve  is  evaluated  using  a  binary
search  for  the  correct  interval  for  the  strain  rate.    The  binary
search is slower than the default incremental search, but in cases
where  large  changes  in  the  strain  rate  may  occur  over  a  single
time  step,  it  is  more  robust.    This  option  is  not  necessary  for  the
viscoplastic formulation.  
LCSR
*MAT_PIECEWISE_LINEAR_PLASTICITY 
DESCRIPTION
VP 
Formulation for rate effects: 
EQ.-1.0:  Cowper-Symonds  with  deviatoric  strain  rate  rather 
than total, 
EQ.0.0:  Scale yield stress (default), 
EQ.1.0:  Viscoplastic formulation. 
EPS1 - EPS8 
Effective plastic strain values (optional; supersedes SIGY, ETAN). 
At least 2 points should be defined.  The first point must be zero
corresponding  to  the  initial  yield  stress.    WARNING:  If  the  first
point is nonzero the yield stress is extrapolated to determine the
initial  yield.    If  this  option  is  used  SIGY  and  ETAN  are  ignored 
and may be input as zero. 
ES1 - ES8 
Corresponding yield stress values to EPS1 - EPS8. 
Remarks: 
The  stress  strain  behavior  may  be  treated  by  a  bilinear  stress  strain  curve  by  defining 
the tangent modulus, ETAN.  Alternately, a curve of effective stress vs.  effective plastic 
strain  similar  to  that  shown  in  Figure  M10-1  may  be  defined  by  (EPS1, ES1)  - 
(EPS8, ES8);  however,  a  curve  ID  (LCSS)  may be  referenced  instead  if  eight  points  are 
insufficient.  The cost is roughly the same for either approach.  Note that in the special 
case of uniaxial stress, true stress vs.  true plastic strain is equivalent to effective stress 
vs.    effective  plastic  strain.    The  most  general  approach  is  to  use  the  table  definition 
(LCSS) discussed below. 
Three options to account for strain rate effects are possible. 
1.  Strain rate may be accounted for using the Cowper and Symonds model which 
scales the yield stress with the factor 
1 + (
𝑝⁄
)
𝜀̇
where 𝜀̇ is the strain rate.  𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗.  If VP = -1.  The deviatoric strain rates are 
used instead. 
If the viscoplastic option is active, VP = 1.0, and if SIGY is > 0 then the dynamic 
𝑝 ),  which  is 
yield  stress  is  computed  from  the  sum  of  the  static  stress,  𝜎𝑦
typically given by a load curve ID, and the initial yield stress, SIGY, multiplied 
by the Cowper-Symonds rate term as follows: 
𝑠(𝜀eff
𝜎𝑦(𝜀eff
𝑝 , 𝜀̇eff
𝑝 ) = 𝜎𝑦
𝑠(𝜀eff
𝑝 ) + SIGY ×
𝑝⁄
𝜀̇eff
⎟⎞
𝐶 ⎠
⎜⎛
⎝
where  the  plastic  strain  rate  is  used.    With  this  latter  approach  similar  results 
can be obtained between this model and material model: *MAT_ANISOTROP-
IC_VISCOPLASTIC.  If SIGY = 0, the following equation is used instead where 
𝑝 ), must be defined by a load curve: 
the static stress, 𝜎𝑦
𝑠(𝜀eff
𝜎𝑦(𝜀eff
𝑝 , 𝜀̇eff
𝑝 ) = 𝜎𝑦
𝑝 )
𝑠(𝜀eff
𝜀̇eff
⎟⎞
𝐶 ⎠
⎜⎛
⎝
⎡
1 +
⎢⎢
⎣
𝑝⁄
⎤
⎥⎥
⎦
This latter equation is always used if the viscoplastic option is off. 
2.  For  complete  generality  a  load  curve  (LCSR)  to  scale  the  yield  stress  may  be 
input instead.  In this curve the scale factor versus strain rate is defined. 
3. 
If different stress versus strain curves can be provided for various strain rates, 
the  option  using  the  reference  to  a  table  (LCSS)  can  be  used.    Then  the  table 
input in *DEFINE_TABLE has to be used, see Figure M24-1. 
A  fully  viscoplastic  formulation  is  optional  (variable  VP)  which  incorporates  the 
different options above within the yield surface.  An additional cost is incurred over the 
simple scaling but the improvement is results can be dramatic. 
For  implicit  calculations  on  this  material  involving  severe  nonlinear  hardening  the 
radial  return  method  may  result  in  inaccurate  stress-strain  response.    By  setting 
IACC = 1  on  *CONTROL_ACCURACY  activates  a  fully  iterative  plasticity  algorithm, 
which  will  remedy  this.    This  is  not  to  be  confused  with  the  MITER  flag  on  *CON-
TROL_SHELL,  which  governs  the  treatment  of  the  plane  stress  assumption  for  shell 
elements.  If failure is applied with this option, incident failure will initiate damage, and 
the  stress  will  continuously  degrade  to  zero  before  erosion  for  a  deformation  of  1% 
plastic  strain.    So  for  instance,  if  the  failure  strain  is  FAIL = 0.05,  then  the  element  is 
eroded  when  𝜀̅𝑝 = 0.06  and  the  material  goes  from  intact  to  completely  damaged 
between  𝜀̅𝑝 = 0.05  and  𝜀̅𝑝 = 0.06.    The  reason  is  to  enhance  implicit  performance  by 
maintaining continuity in the internal forces. 
For  a  nonzero  failure strain,  *DEFINE_MATERIAL_HISTORIES  can  be  used  to  output 
the failure indicator. 
*DEFINE_MATERIAL_HISTORIES Properties 
Label 
Attributes 
Description 
Instability 
- 
- 
- 
- 
Failure indicator 𝜀eff
𝑝 /𝜀fail
𝑝 , see FAIL
*DEFINE_MATERIAL_HISTORIES Properties 
Label 
Attributes 
Description 
Plastic Strain Rate 
- 
- 
- 
- 
𝑝  
Effective plastic strain rate 𝜀̇eff
*MAT_025 
This  is  Material  Type  25.    This  is  an  inviscid  two  invariant  geologic  cap  model.    This 
material model can be used for geomechanical problems or for materials as concrete, see 
references cited below. 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
BULK 
Type 
A8 
  Card 2 
Variable 
Type 
1 
R 
F 
  Card 3 
1 
F 
2 
D 
F 
2 
F 
3 
W 
F 
3 
4 
G 
F 
4 
X0 
F 
4 
Variable 
PLOT 
FTYPE 
VEC 
TOFF 
Type 
F 
F 
F 
F 
5 
6 
7 
8 
ALPHA 
THETA 
GAMMA 
BETA 
F 
5 
C 
F 
5 
F 
6 
N 
F 
6 
F 
7 
F 
8 
7 
8 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density. 
BULK 
Initial bulk modulus, K. 
G 
Initial Shear modulus. 
ALPHA 
THETA 
Failure envelope parameter, α. 
Failure envelope linear coefficient, θ. 
GAMMA 
Failure envelope exponential coefficient, γ.
*MAT_GEOLOGIC_CAP_MODEL 
DESCRIPTION
BETA 
Failure envelope exponent, β. 
R 
D 
W 
X0 
C 
N 
Cap, surface axis ratio. 
Hardening law exponent. 
Hardening law coefficient. 
Hardening law exponent, X0. 
Kinematic hardening coefficient, 𝑐̅. 
Kinematic hardening parameter. 
PLOT 
Save  the  following  variable  for  plotting  in  LS-PrePost,  to  be 
labeled there as “effective plastic strain:” 
EQ.1: hardening parameter, κ 
EQ.2: cap -J1 axis intercept, X(κ) 
𝑝 
EQ.3: volumetric plastic strain 𝜀𝑣
EQ.4: first stress invariant, 𝐽1 
EQ.5: second stress invariant, √𝐽2 
EQ.6: not used 
EQ.7: not used 
EQ.8: response mode number 
EQ.9: number of iterations 
FTYPE 
Formulation flag: 
EQ.1: soils (Cap surface may contract) 
EQ.2: concrete and rock (Cap doesn’t contract) 
VEC 
Vectorization flag: 
EQ.0: vectorized (fixed number of iterations) 
EQ.1: fully iterative 
If the vectorized solution is chosen, the stresses might be slightly
off the yield surface; however, on vector computers a much more
efficient solution is achieved. 
TOFF 
Tension Cut Off, TOFF < 0 (positive in compression).
J2D
J2D = Fe
f1
J2D = Fc
f2
J1
X(κ)
f3
Figure  M25-1.  The  yield  surface  of  the  two-invariant  cap  model  in
pressure√𝐽2𝐷 − 𝐽1 space.  Surface f1 is the failure envelope, f2 is the cap surface,
and f3 is the tension cutoff. 
Remarks: 
The  implementation  of  an  extended  two  invariant  cap  model,  suggested  by  Stojko 
[1990], is based on the formulations of Simo, et al.  [1988, 1990] and Sandler and Rubin 
[1979].    In  this  model,  the  two  invariant  cap  theory  is  extended  to  include  nonlinear 
kinematic  hardening  as  suggested  by  Isenberg,  Vaughan,  and  Sandler  [1978].    A  brief 
discussion of the extended cap model and its parameters is given below.  
The cap model is formulated in terms of the invariants of the stress tensor.  The square 
root  of  the  second  invariant  of  the  deviatoric  stress  tensor,  √𝐽2𝐷  is  found  from  the 
deviatoric stresses s as 
√𝐽2𝐷 ≡ √
𝑆𝑖𝑗𝑆𝑖𝑗 
and  is  the  objective  scalar  measure  of  the  distortional  or  shearing  stress.    The  first 
invariant of the stress, J1, is the trace of the stress tensor. 
The cap model consists of three surfaces in √𝐽2𝐷 − 𝐽1 space, as shown in Figure M25-1  
First, there is a failure envelope surface, denoted f1 in the figure.  The functional form of 
f1 is 
where Fe is given by 
𝑓1 = √𝐽2𝐷 − min[𝐹𝑒(𝐽1), 𝑇mises], 
𝐹𝑒(𝐽1) ≡ 𝛼 − 𝛾exp(−𝛽𝐽1) + 𝜃𝐽1
and  𝑇𝑚𝑖𝑠𝑒𝑠 ≡ |𝑋(𝜅𝑛) − 𝐿(𝜅𝑛)|.    This  failure  envelop  surface  is  fixed  in  √𝐽2𝐷 − 𝐽1  space, 
and therefore does not harden unless kinematic hardening is present.  Next, there is a 
cap surface, denoted f2 in the figure, with f2 given by 
𝑓2 = √𝐽2𝐷 − 𝐹𝑐(𝐽1, 𝐾) 
where Fc is defined by 
𝐹𝑐(𝐽1, 𝜅) ≡
√[𝑋(𝜅) − 𝐿(𝜅)]2 − [𝐽1 − 𝐿(𝜅)]2, 
𝑋(𝜅) is the intersection of the cap surface with the J1 axis 
and 𝐿(𝜅) is defined by  
𝑋(𝜅) = 𝜅 + 𝑅𝐹𝑒(𝜅), 
𝐿(𝜅) ≡ {𝜅   if   𝜅 > 0
0   if   𝜅 ≤ 0
The  hardening  parameter  κ  is  related  to  the  plastic  volume  change  𝜀𝑣
hardening law 
𝑝  through  the 
𝑝 = 𝑊{1 − exp[−𝐷(𝑋(𝜅) − 𝑋0)]} 
𝜀𝑣
Geometrically, κ is seen in the figure as the J1 coordinate of the intersection of the cap 
surface and the failure surface.  Finally, there is the tension cutoff surface, denoted f3 in 
the figure.  The function f3 is given by  
f3 ≡ T − J1 
where  T  is  the  input  material  parameter  which  specifies  the  maximum  hydrostatic 
tension  sustainable  by  the  material.    The  elastic  domain  in  √𝐽2𝐷 − 𝐽1  space  is  then 
bounded  by  the  failure  envelope  surface  above,  the  tension  cutoff  surface  on  the  left, 
and the cap surface on the right. 
An additive decomposition of the strain into elastic and plastic parts is assumed: 
𝜺 = 𝜺𝑒 + 𝜺𝑝, 
where εe is the elastic strain and εp is the plastic strain.  Stress is found from the elastic 
strain using Hooke’s law, 
where σ is the stress and C is the elastic constitutive tensor. 
𝝈 = 𝑪(𝜺  − 𝜺𝒑), 
The yield condition may be written 
𝑓1(𝑠) ≤ 0 
𝑓2(𝑠, 𝜅) ≤ 0 
𝑓3(𝑠) ≤ 0 
and the plastic consistency condition requires that
𝜆̇𝑘𝑓𝑘 = 0 
𝑘 = 1,2,3 
𝜆̇𝑘 ≥ 0 
where 𝜆𝑘 is the plastic consistency parameter for surface k.  If 𝑓𝑘 < 0 then, 𝜆̇𝑘 = 0 and the 
response  is  elastic.    If  𝑓𝑘 > 0  then  surface  k  is  active  and  𝜆̇𝑘  is  found  from  the 
requirement that 𝑓 ̇
𝑘 = 0. 
Associated plastic flow is assumed, so using Koiter’s flow rule the plastic strain rate is 
given as the sum of contribution from all of the active surfaces, 
𝜀̇𝑝 = ∑ 𝜆̇𝑘
𝑘=1
∂𝑓𝑘
∂𝑠
. 
One of the major advantages of the cap model over other classical pressure-dependent 
plasticity models is the ability to control the amount of dilatancy produced under shear 
loading.    Dilatancy  is  produced  under  shear  loading  as  a  result  of  the  yield  surface 
having  a  positive  slope  in  √𝐽2𝐷 − 𝐽  space,  so  the  assumption  of  plastic  flow  in  the 
direction  normal  to  the  yield  surface  produces  a  plastic  strain  rate  vector  that  has  a 
component in the volumetric (hydrostatic) direction .  In models such 
as  the  Drucker-Prager  and  Mohr-Coulomb,  this  dilatancy  continues  as  long  as  shear 
loads are applied, and in many cases produces far more dilatancy than is experimental-
ly  observed  in  material  tests.    In  the  cap  model,  when  the  failure  surface  is  active, 
dilatancy  is  produced  just  as  with  the  Drucker-Prager  and  Mohr-Coulumb  models.  
However, the hardening law permits the cap surface to contract until the cap intersects 
the  failure  envelope  at  the  stress  point,  and  the  cap  remains  at  that  point.    The  local 
normal to the yield surface is now vertical, and therefore the normality rule assures that 
no further plastic volumetric strain (dilatancy) is created.  Adjustment of the parameters 
that  control  the  rate  of  cap  contractions  permits  experimentally  observed  amounts  of 
dilatancy  to  be  incorporated  into  the  cap  model,  thus  producing  a  constitutive  law 
which better represents the physics to be modeled. 
Another advantage of the cap model over other models such as the Drucker-Prager and 
Mohr-Coulomb  is  the  ability  to  model  plastic  compaction.    In  these  models  all  purely 
volumetric response is elastic.  In the cap model, volumetric response is elastic until the 
stress  point  hits  the  cap  surface.    Therefore,  plastic  volumetric  strain  (compaction)  is 
generated at a rate controlled by the hardening law.  Thus, in addition to controlling the 
amount  of  dilatancy,  the  introduction  of  the  cap  surface  adds  another  experimentally 
observed response characteristic of geological material into the model. 
The  inclusion  of  kinematic  hardening  results  in  hysteretic  energy  dissipation  under 
cyclic loading conditions.  Following the approach of Isenberg, et al.  [1978] a nonlinear 
kinematic hardening law is used for the failure envelope surface when nonzero values 
of and N are specified.  In this case, the failure envelope surface is replaced by a family
of  yield  surfaces  bounded  by  an  initial  yield  surface  and  a  limiting  failure  envelope 
surface.  Thus, the shape of the yield surfaces described above remains unchanged, but 
they may translate in a plane orthogonal to the J axis, 
Translation of the yield surfaces is permitted through the introduction of a “back stress” 
tensor,  α  The  formulation  including  kinematic  hardening  is  obtained  by  replacing  the 
stress    σ  with  the  translated  stress  tensor  𝜂 ≡ 𝜎 − 𝛼  in  all  of  the  above  equation.    The 
history  tensor  α  is  assumed  deviatoric,  and  therefore  has  only  5  unique  components.  
The evolution of the back stress tensor is governed by the nonlinear hardening law 
𝛼 = 𝑐 ̅𝐹̅(𝜎, 𝛼)𝑒 ̇𝑝 
where 𝑐 ̅  is  a  constant,  𝐹̅  is  a  scalar  function  of  σ  and  α  and  𝑒 ̇𝑝  is  the  rate  of  deviatoric 
plastic strain.  The constant may be estimated from the slope of the shear stress - plastic 
shear strain curve at low levels of shear stress. 
The function 𝐹̅ is defined as 
𝐹̅ ≡ max [0,1 −
(𝜎 − 𝛼)𝛼
2𝑁𝐹𝑒(𝐽1)
] 
where  N  is  a  constant  defining  the  size  of  the  yield  surface.    The  value  of  N  may  be 
interpreted as the radial distant between the outside of the initial yield surface and the 
inside of the limit surface.  In order for the limit surface of the kinematic hardening cap 
model  to  correspond with  the  failure  envelope  surface  of  the  standard  cap  model,  the 
scalar parameter α must be replaced  α - N in the definition Fe. 
The  cap  model  contains  a  number  of  parameters  which  must  be  chosen  to represent  a 
particular material, and are generally based on experimental data.  The parameters α, β, 
θ, and γ are usually evaluated by fitting a curve through failure data taken from a set of 
triaxial compression tests.  The parameters W, D, and X0 define the cap hardening law.  
The  value  W  represents  the  void  fraction of the  uncompressed  sample  and  D  governs 
the slope of the initial loading curve in hydrostatic compression.  The value of R is the 
ration of major to minor axes of the quarter ellipse defining the cap surface.  Additional 
details and guidelines for fitting the cap model to experimental data are found in Chen 
and Baladi [1985].
*MAT_026 
This  is Material  Type 26.    The  major  use  of this  material  model  is for  honeycomb  and 
foam  materials  with  real  anisotropic  behavior.    A  nonlinear  elastoplastic  material 
behavior  can  be  defined  separately  for  all  normal  and  shear  stresses.    These  are 
considered to be fully uncoupled.  See notes below. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
SIGY 
F 
6 
VF 
F 
7 
8 
MU 
BULK 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
.05 
0.0 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCA 
LCB 
LCC 
LCS 
LCAB 
LCBC 
LCCA 
LCSR 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
LCA 
LCA 
LCA 
LCS 
LCS 
LCS 
optional
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EAAU 
EBBU 
ECCU 
GABU 
GBCU 
GCAU 
AOPT 
MACF 
Type 
F 
F 
F 
F 
F 
F 
  Card 4 
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
3 
ZP 
F 
4 
A1 
F 
5 
A2 
F 
6 
A3 
F 
I 
8
Variable 
1 
D1 
Type 
F 
*MAT_HONEYCOMB 
2 
D2 
F 
3 
D3 
F 
4 
5 
TSEF 
SSEF 
F 
F 
6 
V1 
F 
7 
V2 
F 
8 
V3 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus for compacted honeycomb material. 
Poisson’s ratio for compacted honeycomb material. 
SIGY 
Yield stress for fully compacted honeycomb. 
VF 
MU 
Relative volume at which the honeycomb is fully compacted. 
μ, material viscosity coefficient.  (default=.05)  Recommended. 
BULK 
Bulk viscosity flag: 
LCA 
LCB 
LCC 
LCS 
EQ.0.0: bulk viscosity is not used.  This is recommended. 
EQ.1.0: bulk viscosity is active and μ = 0.  This will give results 
identical to previous versions of LS-DYNA. 
Load curve ID, see *DEFINE_CURVE, for sigma-aa versus either 
relative volume or volumetric strain.  See notes below. 
Load curve ID, see *DEFINE_CURVE, for sigma-bb versus either 
relative  volume  or  volumetric  strain.    Default  LCB = LCA.    See 
notes below. 
Load  curve  ID,  see  *DEFINE_CURVE,  for  sigma-cc  versus  either 
relative  volume  or  volumetric  strain.    Default  LCC = LCA.    See 
notes below. 
Load  curve  ID,  see  *DEFINE_CURVE,  for  shear  stress  versus 
either  relative  volume  or  volumetric  strain.    Default  LCS = LCA. 
Each component of shear stress may have its own load curve.  See
notes below.
VARIABLE   
LCAB 
LCBC 
LCCA 
LCSR 
EAAU 
EBBU 
ECCU 
GABU 
GBCU 
GCAU 
AOPT 
DESCRIPTION
Load curve ID, see *DEFINE_CURVE, for sigma-ab versus either 
relative  volume  or  volumetric  strain.    Default  LCAB = LCS.    See 
notes below. 
Load curve ID, see *DEFINE_CURVE, for sigma-bc versus either 
relative  volume  or  volumetric  strain.    Default  LCBC = LCS.    See 
notes below. 
Load  curve  ID,  see  *DEFINE_CURVE,  or  sigma-ca  versus  either 
relative  volume  or  volumetric  strain.    Default  LCCA = LCS.    See 
notes below. 
Load  curve  ID,  see  *DEFINE_CURVE,  for  strain-rate  effects 
defining the scale factor versus strain rate.  This is optional.  The
curves defined above are scaled using this curve. 
Elastic modulus Eaau in uncompressed configuration. 
Elastic modulus Ebbu in uncompressed configuration. 
Elastic modulus Eccu in uncompressed configuration. 
Shear modulus Gabu in uncompressed configuration. 
Shear modulus Gbcu in uncompressed configuration. 
Shear modulus Gcau in uncompressed configuration. 
Material  axes  option  : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by 
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES. 
EQ.1.0: locally orthotropic with material axes determined by a
point  in  space  and  the  global  location  of  the  element
center; this is the a-direction. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element 
defined  by  the  cross  product  of  the  vector  v  with  the
*MAT_HONEYCOMB 
DESCRIPTION
element  normal.    The  plane  of  a  solid  element  is  the
midsurface between the inner surface and outer surface
defined by the first four nodes and the last four nodes 
of the connectivity of the element, respectively. 
EQ.4.0: locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector  v,  and
an originating point, p, which define the centerline ax-
is.  This option is for solid elements only. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later.. 
MACF 
Material axes change flag: 
EQ.1: No change, default, 
EQ.2: switch material axes a and b, 
EQ.3: switch material axes a and c, 
EQ.4: switch material axes b and c. 
XP YP ZP 
Coordinates of point p for AOPT = 1 and 4. 
A1 A2 A3 
Components of vector a for AOPT = 2. 
D1 D2 D3 
Components of vector d for AOPT = 2. 
V1 V2 V3 
Define components of vector v for AOPT = 3 and 4. 
Tensile strain at element failure (element will erode). 
Shear strain at element failure (element will erode). 
TSEF 
SSEF 
Remarks: 
For  efficiency  it  is  strongly  recommended  that  the  load  curve  ID’s:  LCA,  LCB,  LCC, 
LCS,  LCAB,  LCBC,  and  LCCA,  contain  exactly  the  same  number  of  points  with 
corresponding  strain  values  on  the  abscissa.    If  this  recommendation  is  followed  the 
cost  of  the  table  lookup  is  insignificant.    Conversely,  the  cost  increases  significantly  if 
the abscissa strain values are not consistent between load curves.
The  behavior  before  compaction  is  orthotropic  where  the  components  of  the  stress 
tensor are uncoupled, i.e., an a component of strain will generate resistance in the local 
a-direction  with  no  coupling  to  the  local  b  and  c  directions.    The  elastic  moduli  vary, 
from  their  initial  values  to  the  fully  compacted  values  at  Vf,  linearly  with  the  relative 
volume V: 
𝐸𝑎𝑎 = 𝐸𝑎𝑎𝑢 + 𝛽(𝐸 − 𝐸𝑎𝑎𝑢) 
𝐸𝑏𝑏 = 𝐸𝑏𝑏𝑢 + 𝛽(𝐸 − 𝐸𝑏𝑏𝑢) 
𝐸𝑐𝑐 = 𝐸𝑐𝑐𝑢 + 𝛽(𝐸 − 𝐸𝑐𝑐𝑢) 
𝐺𝑎𝑏 = 𝐸𝑎𝑏𝑢 + 𝛽(𝐺 − 𝐺𝑎𝑏𝑢) 
𝐺𝑏𝑐 = 𝐸𝑏𝑐𝑢 + 𝛽(𝐺 − 𝐺𝑏𝑐𝑢) 
𝐺𝑐𝑎 = 𝐸𝑐𝑎𝑢 + 𝛽(𝐺 − 𝐺𝑐𝑎𝑢) 
𝛽 = max [min (
1 − 𝑉
1 − 𝑉𝑓
, 1) , 0] 
where 
and G is the elastic shear modulus for the fully compacted honeycomb material 
𝐺 =
2(1 + 𝑣)
. 
The  relative  volume,  V,  is  defined  as  the  ratio  of  the  current  volume  to  the  initial 
volume.    Typically,  V = 1  at  the  beginning  of  a  calculation.    The  viscosity  coefficient  µ 
(MU) should be set to a small number (usually .02 - .10 is okay).  Alternatively, the two 
bulk viscosity coefficients on the control cards should  be set to very small numbers to 
prevent  the  development  of  spurious  pressures  that  may  lead  to  undesirable  and 
confusing results.  The latter is not recommended since spurious numerical noise may 
develop.
Curve extends into negative volumetric 
strain quadrant since LS-DYNA will 
extrapolate using the two end points. It 
is important that the extropolation 
does not extend into the negative 
 σ
ij
unloading and
reloading path
Strain: -ε
ij
Unloading is based on the interpolated Young’s 
moduli which must provide an unloading tangent 
that exceeds the loading tangent.
Figure  M26-1.    Stress  quantity  versus  volumetric  strain.  Note that  the  “yield
stress” at a volumetric strain of zero is non-zero.  In the load curve definition,
see  *DEFINE_CURVE,  the  “time”  value  is  the  volumetric  strain  and  the
“function” value is the yield stress. 
The  load  curves  define  the  magnitude  of  the  average  stress  as  the  material  changes 
density  (relative  volume),  see  Figure  M26-1.    Each  curve  related  to  this  model  must 
have the same number of points and the same abscissa values.  There are two ways to 
define  these  curves,  a)  as  a  function  of  relative  volume  (V)  or  b)  as  a  function  of 
volumetric strain defined as: 
𝜀𝑉 = 1 − 𝑉 
In  the  former,  the  first  value  in  the  curve  should  correspond  to  a  value  of  relative 
volume slightly less than the fully compacted value.  In the latter, the first value in the 
curve should be less than or equal to zero, corresponding to tension, and increase to full 
compaction.  Care  should  be  taken  when  defining  the  curves  so  that  extrapolated 
values do not lead to negative yield stresses. 
At  the  beginning  of  the  stress  update  each  element’s  stresses  and  strain  rates  are 
transformed  into  the  local  element  coordinate  system.    For  the  uncompacted  material, 
the trial stress components are updated using the elastic interpolated moduli according 
to: 
𝑛+1trial
𝜎𝑎𝑎
𝑛+1trial
𝜎𝑏𝑏
𝑛+1trial
𝜎𝑐𝑐
𝑛+1trial
𝜎𝑎𝑏
= 𝜎𝑎𝑎
= 𝜎𝑏𝑏
= 𝜎𝑐𝑐
= 𝜎𝑎𝑏
𝑛 + 𝐸𝑎𝑎Δ𝜀𝑎𝑎 
𝑛 + 𝐸𝑏𝑏Δ𝜀𝑏𝑏 
𝑛 + 𝐸𝑐𝑐Δ𝜀𝑐𝑐 
𝑛 + 2𝐺𝑎𝑏Δ𝜀𝑎𝑏
𝑛+1trial
𝜎𝑏𝑐
= 𝜎𝑏𝑐
𝑛 + 2𝐺𝑏𝑐Δ𝜀𝑏𝑐 
𝑛+1trial
𝜎𝑐𝑎
= 𝜎𝑐𝑎
𝑛 + 2𝐺𝑐𝑎Δ𝜀𝑐𝑎 
Each  component  of  the  updated  stresses  is  then  independently  checked  to  ensure  that 
they do not exceed the permissible values determined from the load curves; e.g., if 
then 
𝑛+1trial
∣𝜎𝑖𝑗
∣ > 𝜆𝜎𝑖𝑗(𝑉) 
𝑛+1 = 𝜎𝑖𝑗(𝑉)
𝜎𝑖𝑗
𝑛+1trial
𝜆𝜎𝑖𝑗
∣𝜆𝜎𝑖𝑗
𝑛+1trial∣
On  Card  2  σij  (V)  is  defined  by  LCA  for  the  aa  stress  component,  LCB  for  the  bb 
component,  LCC  for  the  cc  component,  and  LCS  for  the  ab,  bc,  ca  shear  stress 
components.    The  parameter  λ  is  either  unity  or  a  value  taken  from  the  load  curve 
number, LCSR, that defines λ as a function of strain-rate.  Strain-rate is defined here as 
the Euclidean norm of the deviatoric strain-rate tensor. 
For fully compacted material it is assumed that the material behavior is elastic-perfectly 
plastic and the stress components updated according to: 
where the deviatoric strain increment is defined as 
trial = 𝑠𝑖𝑗
𝑠𝑖𝑗
𝑑𝑒𝑣
𝑛 + 2𝐺Δ𝜀𝑖𝑗
𝑛+1
2⁄
Δ𝜀𝑖𝑗
dev = Δ𝜀𝑖𝑗 −
Δ𝜀𝑘𝑘𝛿𝑖𝑗 
Now  a  check  is  made  to  see  if  the  yield  stress  for  the  fully  compacted  material  is 
exceeded by comparing  
trial = (
𝑠eff
2⁄
trial)
trial𝑠𝑖𝑗
𝑠𝑖𝑗
the  effective  trial  stress  to  the  defined  yield  stress,  SIGY.    If  the  effective  trial  stress 
exceeds  the  yield  stress  the  stress  components  are  simply  scaled  back  to  the  yield 
surface 
Now the pressure is updated using the elastic bulk modulus, K 
𝑛+1 =
𝑠𝑖𝑗
𝜎𝑦
trial
𝑠eff
trial. 
𝑠𝑖𝑗
where 
𝑛+1
𝑝𝑛+1 = 𝑝𝑛 − 𝐾Δ𝜀𝑘𝑘
2⁄
𝐾 =
3(1 − 2𝑣)
to obtain the final value for the Cauchy stress 
𝑛+1 = 𝑠𝑖𝑗
𝜎𝑖𝑗
𝑛+1 − 𝑝𝑛+1𝛿𝑖𝑗 
After  completing  the  stress  update  transform  the  stresses  back  to  the  global 
configuration. 
For  *CONSTRAINED_TIED_NODES_WITH_FAILURE,  the  failure  is  based  on  the 
volume strain instead to the plastic strain.
*MAT_MOONEY-RIVLIN_RUBBER 
This is Material Type 27.  A two-parametric material model for rubber can be defined. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
Variable 
SGL 
SW 
Type 
F 
F 
3 
PR 
F 
3 
ST 
F 
4 
A 
F 
4 
LCID 
F 
5 
B 
F 
5 
6 
REF 
F 
6 
7 
8 
7 
8 
  VARIABLE   
DESCRIPTION
MID 
RO 
PR 
A 
B 
REF 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Poisson’s  ratio  (value  between  0.49  and  0.5  is  recommended,
smaller values may not work). 
Constant, see literature and equations defined below. 
Constant, see literature and equations defined below. 
Use  reference  geometry  to  initialize  the  stress  tensor.    The
reference geometry is defined by the keyword:*INITIAL_FOAM_-
REFERENCE_GEOMETRY . 
EQ.0.0: off, 
EQ.1.0: on. 
If  the  values  on  Card  2  are  nonzero,  then  a  least  squares  fit  is  computed  from  the
uniaxial data provided by the curve LCID superceding the A and B values on Card 1.
If  the  A  and  B  fields  are  left  blank  on  Card  1  then  the  variables  on  Card  2  must  be 
nonzero. 
SGL 
Specimen gauge length 𝑙0, see Figure M27-1.
*MAT_MOONEY-RIVLIN_RUBBER 
DESCRIPTION
Specimen width, see Figure M27-1. 
Specimen thickness, see Figure M27-1. 
Curve  ID,  see  *DEFINE_CURVE,  giving  the  force  versus  actual 
change  𝐿  in  the  gauge  length.    See  also  Figure  M27-2  for  an 
alternative definition. 
*MAT_027 
  VARIABLE   
SW 
ST 
LCID 
Remarks: 
The strain energy density function is defined as: 
𝑊 = 𝐴(𝐼 − 3) + 𝐵(𝐼𝐼 − 3) + 𝐶(𝐼𝐼𝐼−2 − 1) + 𝐷(𝐼𝐼𝐼 − 1)2 
where 
𝐶 = 0.5𝐴 + 𝐵 
𝐷 =
𝐴(5𝜐 − 2) + 𝐵(11𝜐 − 5)
2(1 − 2𝜐)
𝜈 =  Poisson’s ratio 
2(𝐴 + 𝐵) = shear modulus of linear elasticity 
𝐼, 𝐼𝐼, 𝐼𝐼𝐼 =  invariants of right Cauchy-Green Tensor C. 
The  load  curve  definition  that  provides  the  uniaxial  data  should  give  the  change  in 
gauge  length,  Δ𝐿,  versus  the  corresponding  force.    In  compression  both  the  force  and 
the  change  in  gauge  length  must  be  specified  as  negative  values.    In  tension  the  force 
and  change  in  gauge  length  should  be  input  as  positive  values.    The  principal  stretch 
ratio in the uniaxial direction, 𝜆1, is then given by 
𝐿0 + Δ𝐿
𝐿0
𝜆1 =
with 𝐿0 being the initial length and 𝐿 being the actual length. 
Alternatively,  the  stress  versus  strain  curve  can  also  be  input  by  setting  the  gauge 
length, thickness, and width to unity (1.0) and defining the engineering strain in place 
of the change in gauge length and the nominal (engineering) stress in place of the force, 
see Figure M27-1. 
The least square fit to the experimental data is performed during the initialization phase 
and is a comparison between the fit and the actual input is provided in the d3hsp file.  
It is a good idea to visually check to make sure it is acceptable.  The coefficients 𝐴 and 𝐵 
are  also  printed  in  the  output  file.    It  is  also  advised  to  use  the  material  driver   for checking out the material model.
gauge
length
Force
AA
Δ gauge length
Section AA
thickness
width
Figure M27-1.  Uniaxial specimen for experimental data 
applied force
initial area
=
A0
change in gauge length
gauge length
=
∆L
Figure  M27-2    The  stress  versus  strain  curve  can  used  instead  of  the  force
versus  the  change  in  the  gauge  length  by  setting  the  gauge  length,  thickness,
and  width  to  unity  (1.0)  and  defining  the  engineering  strain  in  place  of  the
change  in  gauge  length  and  the  nominal  (engineering)  stress  in  place  of  the
force.  *MAT_077_O is a better alternative for fitting data resembling the curve
above.    *MAT_027  will  provide  a  poor  fit  to  a  curve  that  exhibits  an  strong
upturn in slope as strains become large.
*MAT_RESULTANT_PLASTICITY 
This  is  Material  Type  28.    A  resultant  formulation  for  beam  and  shell  elements 
including  elasto-plastic  behavior  can  be  defined.    This  model  is  available  for  the 
Belytschko-Schwer  beam,  the  Co  triangular  shell,  the  Belytschko-Tsay  shell,  and  the 
fully  integrated  type  16  shell.    For  beams,  the  treatment  is  elastic-perfectly  plastic,  but 
for  shell  elements  isotropic  hardening  is  approximately  modeled.    For  a  detailed 
description  we  refer  to  the  LS-DYNA  Theory  Manual.    Since  the  stresses  are  not 
computed  in  the  resultant  formulation,  the  stresses  output  to  the  binary  databases  for 
the resultant elements are zero. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
6 
7 
8 
SIGY 
ETAN 
F 
F 
Default 
none 
none 
none 
none 
none 
0.0 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
SIGY 
ETAN 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s modulus 
Poisson’s ratio 
Yield stress 
Plastic hardening modulus (for shells only)
*MAT_029 
This  is  Material  Type  29.    With  this  material  model,  for  the  Belytschko-Schwer  beam 
only,  plastic  hinge  forming  at  the  ends  of  a  beam  can  be  modeled  using  curve 
definitions.  Optionally, collapse can also be modeled.  See also *MAT_139. 
Description:  FORCE LIMITED Resultant Formulation 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
DF 
F 
6 
7 
8 
AOPT 
YTFLAG 
ASOFT 
F 
F 
F 
Default 
none 
none 
none 
none 
0.0 
0.0 
0.0 
0.0 
  Card 2 
1 
Variable 
M1 
Type 
F 
Default 
none 
  Card 3 
1 
2 
M2 
F 
0 
2 
3 
M3 
F 
0 
3 
4 
M4 
F 
0 
4 
5 
M5 
F 
0 
5 
6 
M6 
F 
0 
6 
7 
M7 
F 
0 
7 
8 
M8 
F 
0 
8 
Variable 
LC1 
LC2 
LC3 
LC4 
LC5 
LC6 
LC7 
LC8 
Type 
F 
Default 
none 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LPS1 
SFS1 
LPS2 
SFS2 
YMS1 
YMS2 
Type 
Default 
F 
0 
F 
F 
F 
F 
F 
1.0 
LPS1 
1.0 
1.0E+20 YMS1 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LPT1 
SFT1 
LPT2 
SFT2 
YMT1 
YMT2 
Type 
Default 
F 
0 
F 
F 
F 
F 
F 
1.0 
LPT1 
1.0 
1.0E+20 YMT1 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LPR 
SFR 
YMR 
Type 
Default 
F 
0 
F 
F 
1.0 
1.0E+20
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
DF 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s modulus 
Poisson’s ratio 
Damping  factor, see definition in  notes below.  A proper control
for the timestep has to be maintained by the user!
VARIABLE   
DESCRIPTION
AOPT 
Axial load curve option: 
EQ.0.0: axial load curves are force versus strain, 
EQ.1.0: axial load curves are force versus change in length. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
YTFLAG 
Flag to allow beam to yield in tension: 
EQ.0.0: beam does not yield in tension, 
EQ.1.0: beam can yield in tension. 
ASOFT 
M1, M2, 
…, M8 
LC1, LC2, 
…, LC8 
LPS1 
SFS1 
LPS2 
SFS2 
YMS1 
Axial  elastic  softening  factor  applied  once  hinge  has  formed.
When a hinge has formed the stiffness is reduced by this factor.  If
zero, this factor is ignored. 
Applied  end  moment  for  force  versus  (strain/change  in  length)
curve.  At least one must be defined.  A maximum of 8 moments
can be defined.  The values should be in ascending order. 
Load  curve  ID    defining  axial  force 
(collapse load) versus strain/change in length  for the
corresponding applied end moment.  Define the same number as
end  moments.    Each  curve  must  contain  the  same  number  of
points. 
Load curve ID for plastic moment versus rotation about s-axis at 
node 1.  If zero, this load curve is ignored. 
Scale factor for plastic moment versus rotation curve about s-axis 
at node 1.  Default = 1.0. 
Load curve ID for plastic moment versus rotation about s-axis at 
node 2.  Default: is same as at node 1. 
Scale factor for plastic moment versus rotation curve about s-axis 
at node 2.  Default: is same as at node 1. 
Yield  moment  about  s-axis  at  node  1  for  interaction  calculations 
(default set to 1.0E+20 to prevent interaction).
*MAT_FORCE_LIMITED 
DESCRIPTION
Yield  moment  about  s-axis  at  node  2  for  interaction  calculations 
(default set to YMS1). 
Load curve ID for plastic moment versus rotation about t-axis at 
node 1.  If zero, this load curve is ignored. 
Scale factor for plastic moment versus rotation curve about t-axis 
at node 1.  Default = 1.0. 
Load curve ID for plastic moment versus rotation about t-axis at 
node 2.  Default: is the same as at node 1. 
Scale factor for plastic moment versus rotation curve about t-axis 
at node 2.  Default: is the same as at node 1. 
Yield  moment  about  t-axis  at  node  1  for  interaction  calculations 
(default set to 1.0E+20 to prevent interactions) 
Yield  moment  about  t-axis  at  node  2  for  interaction  calculations 
(default set to YMT1) 
Load  curve  ID  for  plastic  torsional  moment  versus  rotation.    If
zero, this load curve is ignored. 
Scale  factor  for  plastic  torsional  moment  versus  rotation
(default = 1.0). 
Torsional yield moment for interaction calculations (default set to
1.0E+20 to prevent interaction) 
YMS2 
LPT1 
SFT1 
LPT2 
SFT2 
YMT1 
YMT2 
LPR 
SFR 
YMR 
Remarks: 
This material model is available for the Belytschko resultant beam element only.  Plastic 
hinges form at the ends of the beam when the moment reaches the plastic moment.  The 
moment versus rotation relationship is specified by the user in the form of a load curve 
and  scale  factor.    The  points  of  the  load  curve  are  (plastic  rotation  in  radians,  plastic 
moment).    Both  quantities  should  be  positive  for  all  points,  with  the  first  point  being 
(zero, initial plastic moment).  Within this constraint any form of characteristic may be 
used,  including  flat  or  falling  curves.    Different  load  curves  and  scale  factors  may  be 
specified at each node and about each of the local s and t axes. 
Axial  collapse  occurs  when  the  compressive  axial  load  reaches  the  collapse  load.  
Collapse  load  versus  collapse  deflection  is  specified  in  the  form  of  a  load  curve.    The 
points  of  the  load  curve  are  either  (true  strain,  collapse  force)  or  (change  in  length,
collapse force).  Both quantities should be entered as positive for all points, and will be 
interpreted as compressive.  The first point should be (zero, initial collapse load). 
The collapse load may vary with end moment as well as with deflections.  In this case 
several  load-deflection  curves  are  defined,  each  corresponding  to  a  different  end 
moment.    Each  load  curve  should  have  the  same  number  of  points  and  the  same 
deflection values.  The end moment is defined as the average of the absolute moments 
at each end of the beam and is always positive. 
Stiffness-proportional  damping  may  be  added  using  the  damping  factor  λ.    This  is 
defined as follows: 
𝜆 =
2 × 𝜉
where ξ is the damping factor at the reference frequency ω (in radians per second).  For 
example if 1% damping at 2Hz is required 
𝜆 =
2 × 0.01
2𝜋 × 2
= 0.001592 
If damping is used, a small timestep may be required.  LS-DYNA does not check this so 
to  avoid  instability  it may  be  necessary  to  control  the  timestep via  a  load  curve.   As a 
guide,  the  timestep  required  for  any  given  element  is  multiplied  by  0.3L⁄cλ  when 
damping is present (L = element length, c = sound speed). 
Moment Interaction: 
Plastic  hinges  can  form  due  to  the  combined  action  of  moments  about  the  three  axes.  
This facility is activated only when yield moments are defined in the material input.  A 
hinge forms when the following condition is first satisfied. 
where, 
⎜⎛ 𝑀𝑟
⎟⎞
𝑀ryield⎠
⎝
+
⎜⎛ 𝑀𝑠
⎟⎞
𝑀syield⎠
⎝
+
⎜⎛ 𝑀𝑡
⎟⎞
𝑀tyield⎠
⎝
≥ 1 
𝑀𝑟,  𝑀𝑠,  𝑀𝑡, = current moment 
𝑀𝑟yield, 𝑀𝑠yield, 𝑀𝑡yield = yield moment 
Note that scale factors for hinge behavior defined in the input will also be applied to the 
yield  moments:    for  example,  𝑀𝑠yield  in  the  above  formula  is  given  by  the  input  yield 
moment about the local axis times the input scale factor for the local s axis.  For strain-
softening  characteristics,  the  yield  moment  should  generally  be  set  equal  to  the  initial 
peak of the moment-rotation load curve. 
On forming a hinge, upper limit moments are set.  These are given by
M8
M7
M6
M5
M4
M3
M2
M1M1
Strain (or change in length, see AOPT)
Figure  M29-1.    The  force  magnitude  is  limited  by  the  applied  end  moment.
For an intermediate value of the end moment LS-DYNA interpolates between 
the curves to determine the allowable force value. 
𝑀𝑟upper = max
⎜⎛𝑀𝑟,
⎝
𝑀𝑟yield
⎟⎞ 
2 ⎠
and similar conditions hold for 𝑀𝑠upper and 𝑀𝑡upper. 
Thereafter, the plastic moments will be given by 
𝑀𝑟𝑝 = min(𝑀𝑟upper, 𝑀𝑟curve) 
where, 
𝑀𝑟p = current plastic moment 
𝑀𝑟curve = moment from load curve at the current rotation scaled by the scale factor.
𝑀𝑠𝑝and 𝑀𝑡𝑝 satisfy similar conditions. 
The  effect  of  this  is  to  provide  an  upper  limit  to  the  moment  that can  be  generated;  it 
represents the softening effect of local buckling at a hinge site.  Thus if a member is bent 
about  is  local  s-axis  it  will  then  be  weaker  in  torsion  and  about  its  local  t-axis.    For 
moment-softening curves, the effect is to trim off the initial peak (although if the curves 
subsequently harden, the final hardening will also be trimmed off). 
It is not possible to make the plastic moment vary with axial load.
*MAT_SHAPE_MEMORY 
This  is  material  type  30.      This  material  model  describes  the  superelastic  response 
present in shape-memory alloys (SMA), that is the peculiar material ability to undergo 
large deformations with a full recovery in loading-unloading cycles .  
The material response is always characterized by a hysteresis loop.  See the references 
by Auricchio, Taylor and Lubliner [1997] and Auricchio and Taylor [1997].  This model 
is available for shells, solids, and Hughes-Liu beam elements. 
5 
6 
7 
8 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
Default 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SIG_ASS  SIG_ASF  SIG_SAS  SIG_SAF 
EPSL 
ALPHA 
YMRT 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
0.0 
0.0 
Optional  Load  Curve  Card  (starting  with  R7.1).    Load  curves  for  mechanically 
induced phase transitions. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID_AS  LCID_SA 
Type 
I 
I 
Default 
none 
none
VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
SIG_ASS 
SIG_ASF 
SIG_SAS 
SIG_SAF 
EPSL 
ALPHA 
YMRT 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Density 
Young’s modulus 
Poisson’s ratio 
Starting  value  for  the  forward  phase  transformation  (conversion
of austenite into martensite) in the case of a uniaxial tensile state
of stress.  A load curve for SIG_ASS as a function of temperature 
is specified by using the negative of the load curve ID number. 
Final  value  for  the  forward  phase  transformation  (conversion  of
austenite into martensite) in the case of a uniaxial tensile state of
stress.  SIG_ASF as a function of temperature is specified by using
the negative of the load curve ID number. 
Starting value for the reverse phase transformation (conversion of
martensite into austenite) in the case of a uniaxial tensile state of
stress.  SIG_SAS as a function of temperature is specified by using
the negative of the load curve ID number. 
Final  value  for  the  reverse  phase  transformation  (conversion  of
martensite into austenite) in the case of a uniaxial tensile state of
stress.  SIG_SAF as a function of temperature is specified by using
the negative of the load curve ID number. 
Recoverable strain or maximum residual strain.  It is a measure of
the  maximum  deformation  obtainable  all  the  martensite  in  one
direction. 
Parameter  measuring  the  difference  between  material  responses
in  tension  and  compression  (set  alpha = 0  for  no  difference). 
Also, see the following Remark. 
Young’s  modulus  for  the  martensite  if  it  is  different  from  the
modulus for the austenite.  Defaults to the austenite modulus if it 
is set to zero. 
LCID_AS 
Load  curve  ID  or  Table  ID  for  the  forward  phase  change 
(conversion of austenite into martensite). 
1.  When LCID_AS is a load curve ID the curve is taken to be
*MAT_SHAPE_MEMORY 
DESCRIPTION
effective  stress  versus  martensite  fraction  (ranging  from
0 to 1). 
2.  When  LCID_AS  is  a  table  ID  the  table  defines  for  each 
phase  transition  rate  (derivative  of  martensite  fraction)  a
load  curve  ID  specifying  the  stress  versus  martensite
fraction for that phase transition rate.   
The stress versus martensite fraction curve for the lowest
value  of  the  phase  transition  rate  is  used,  if  the  phase
transition rate falls below the minimum value.  Likewise,
the stress versus martensite fraction curve for the highest
value  of  phase  transition  rate  is  used  if  phase  transition
rate exceeds the maximum value. 
3.  The  values  of  SIG_ASS  and  SIG_ASF  are  overwritten
when this option is used. 
LCID_SA 
Load curve ID or Table ID for reverse phase change (conversion of 
martensite into austenite). 
1.  When LCID_SA is a load curve ID the curve is taken to be 
effective  stress  versus  martensite  fraction  (ranging  from
0 to 1). 
2.  When  LCID_SA  is  a  table  ID  the  table  defines  for  each 
phase  transition  rate  (derivative  of  martensite  fraction)  a 
load  curve  ID  specifying  the  stress  versus  martensite
fraction for that phase transition rate. 
The stress versus martensite fraction curve for the lowest
value  of  the  phase  transition  rate  is  used,  if  the  phase
transition rate falls below the minimum value.  Likewise,
the stress versus martensite fraction curve for the highest
value  of  phase  transition  rate  is  used  if  phase  transition
rate exceeds the maximum value. 
3.  The  values  of  SIG_ASS  and  SIG_ASF  are  overwritten
when this option is used. 
Remarks: 
The material parameter alpha, α, measures the difference between material responses in 
tension  and  compression.    In  particular,  it  is  possible  to  relate  the  parameter  α  to  the
σAX
σAS
σSA
σSA
(cid:3)
(cid:3)L
Figure M30-1.  Superelastic Behavior for a Shape Memory Material 
initial stress value of the austenite into martensite conversion, indicated respectively as 
𝐴𝑆,+ and 𝜎𝑠
𝜎𝑠
𝐴𝑆,−, according to the following expression: 
𝛼 =
𝐴𝑆,− − 𝜎𝑠
𝜎𝑠
𝐴𝑆,− + 𝜎𝑠
𝜎𝑠
𝐴𝑆,+
𝐴𝑆,+
In  the  following,  the  results  obtained  from  a  simple  test  problem  is  reported.    The 
material properties are set as: 
E 
PR 
60000 MPa 
0.3 
SIG_ASS 
520 MPa 
SIG_ASF 
600 MPa 
SIG_SAS 
300 MPa 
SIG_SAF 
200 MPa
1000
500
-500
-1000
-0.1
-0.05
0.05
True Strain
 Figure M30-2.  Complete loading-unloading test in tension and compression.
EPSL 
0.07 
ALPHA 
0.12 
YMRT 
50000 MPa 
The  investigated  problem  is  the  complete  loading-unloading  test  in  tension  and 
compression.    The  uniaxial  Cauchy  stress  versus  the  logarithmic  strain  is  plotted  in 
Figure M30-2.
*MAT_FRAZER_NASH_RUBBER_MODEL 
This  is  Material  Type  31.    This  model  defines  rubber  from  uniaxial  test  data.    It  is  a 
modified form of the hyperelastic constitutive law first described in Kenchington [1988].  
See also the notes below. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
PR 
F 
3 
4 
5 
6 
7 
8 
C100 
C200 
C300 
C400 
F 
4 
F 
5 
F 
6 
F 
7 
8 
Variable 
C110 
C210 
C010 
C020 
EXIT 
EMAX 
EMIN 
REF 
Type 
F 
  Card 3 
1 
F 
2 
Variable 
SGL 
SW 
Type 
F 
F 
F 
3 
ST 
F 
F 
4 
LCID 
F 
F 
5 
F 
6 
F 
7 
F 
8 
  VARIABLE   
DESCRIPTION
MID 
RO 
PR 
C100 
C200 
C300 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Poisson’s ratio.  Values between .49 and .50 are suggested. 
C100 (EQ.1.0 if term is in the least squares fit.) 
C200 (EQ.1.0 if term is in the least squares fit.) 
C300 (EQ.1.0 if term is in the least squares fit.)
C400 
C110 
C210 
C010 
C020 
EXIT 
*MAT_FRAZER_NASH_RUBBER_MODEL 
DESCRIPTION
C400 (EQ.1.0 if term is in the least squares fit.) 
C110 (EQ.1.0 if term is in the least squares fit.) 
C210 (EQ.1.0 if term is in the least squares fit.) 
C010 (EQ.1.0 if term is in the least squares fit.) 
C020 (EQ.1.0 if term is in the least squares fit.) 
Exit option: 
EQ.0.0: stop if strain limits are exceeded (recommended), 
NE.0.0:  continue if strain limits are exceeded.  The curve is then
extrapolated. 
EMAX 
Maximum strain limit, (Green-St, Venant Strain). 
EMIN 
Minimum strain limit, (Green-St, Venant Strain). 
Use  reference  geometry  to  initialize  the  stress  tensor.    The
reference  geometry  is  defined  by  the  keyword:  *INITIAL_-
FOAM_REFERENCE_GEOMETRY . 
EQ.0.0: off, 
EQ.1.0: on. 
Specimen gauge length, see Figure M27-1. 
Specimen width, see Figure M27-1. 
Specimen thickness, see Figure M27-1. 
Load  curve  ID,  see  DEFINE_CURVE,  giving  the  force  versus 
actual  change  in  gauge  length.    See  also  Figure  M27-2  for  an 
alternative definition. 
REF 
SGL 
SW 
ST 
LCID 
Remarks: 
The  constants  can  be  defined  directly  or  a  least  squares  fit  can  be  performed  if  the 
uniaxial data (SGL, SW, ST and LCID) is available.  If a least squares fit is chosen, then 
the  terms  to  be  included  in  the  energy  functional  are  flagged  by  setting  their
corresponding coefficients to unity.  If all coefficients are zero the default is to use only 
the terms involving I1 and I2.  C100 defaults to unity if the least square fit is used. 
The strain energy functional, U, is defined in terms of the input constants as: 
𝑈 = 𝐶100𝐼1 + 𝐶200𝐼1
2 + 𝐶300𝐼1
3 + 𝐶400𝐼1
4 + 𝐶110𝐼1𝐼2 +   𝐶210𝐼1
2𝐼2 + 𝐶010𝐼2 + 𝐶020𝐼2
2 + 𝑓 (𝐽) 
where the invariants can be expressed in terms of the deformation gradient matrix, Fij, 
and the Green-St.  Venant strain tensor, Eij : 
𝐽 = ∣𝐹𝑖𝑗∣ 
𝐼1 = 𝐸𝑖𝑖 
𝐼2 =
2!
𝑖𝑗 𝐸𝑝𝑖𝐸𝑞𝑗 
𝛿𝑝𝑞
The  derivative  of  U  with  respect  to  a  component  of  strain  gives  the  corresponding 
component of stress 
here, Sij, is the second Piola-Kirchhoff stress tensor. 
𝑆𝑖𝑗 =
∂𝑈
∂𝐸𝑖𝑗
The  load  curve  definition  that  provides  the  uniaxial  data  should  give  the  change  in 
gauge length, ΔL, and the corresponding force.  In compression both the force and the 
change in gauge length must be specified as negative values.  In tension the force and 
change in gauge length should be input as positive values.  The principal stretch ratio in 
the uniaxial direction, λ1, is then given by 
𝜆 =
𝐿𝑜 + Δ𝐿
𝐿𝑜
Alternatively,  the  stress  versus  strain  curve  can  also  be  input  by  setting  the  gauge 
length, thickness, and width to unity and defining the engineering strain in place of the 
change  in  gauge  length  and  the  nominal  (engineering)  stress  in  place  of  the  force,  see 
Figure  M27-2  The  least  square  fit  to  the  experimental  data  is  performed  during  the 
initialization phase and is a comparison between the fit and the actual input is provided 
in the printed file.  It is a good idea to visually check the fit to make sure it is acceptable.  
The coefficients C100 - C020 are also printed in the output file.
*MAT_LAMINATED_GLASS 
This is Material Type 32.  With this material model, a layered glass including polymeric 
layers can be modeled.  Failure of the glass part is possible.  See notes below. 
Card 1 
1 
Variable 
MID 
Type 
A8 
Card 2 
1 
2 
RO 
F 
2 
3 
EG 
F 
3 
Variable 
PRP 
SYP 
ETP 
Type 
F 
F 
F 
4 
5 
6 
7 
PRG 
SYG 
ETG 
EFG 
F 
4 
F 
5 
F 
6 
F 
7 
8 
EP 
F 
8 
Integration  Point  Cards.    Define  1-4  cards  specifying  up  to  32  values.    If  less  than  4 
cards are input, reading is stopped by a “*” control card.  
Card 3 
Variable 
1 
F1 
Type 
F 
2 
F2 
F 
3 
F3 
F 
4 
F4 
F 
5 
F5 
F 
6 
F6 
F 
7 
F7 
F 
8 
F8 
F 
VARIABLE 
DESCRIPTION 
MID 
RO 
EG 
PRG 
SYG 
ETG 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s modulus for glass 
Poisson’s ratio for glass 
Yield stress for glass 
Plastic hardening modulus for glass
DESCRIPTION 
*MAT_032 
EFG 
EP 
PRP 
SYP 
ETP 
Plastic strain at failure for glass 
Young’s modulus for polymer 
Poisson’s ratio for polymer 
Yield stress for polymer 
Plastic hardening modulus for polymer 
F1, …, FN 
Integration point material: 
fn = 0.0:  glass, 
fn = 1.0:  polymer. 
A user-defined integration rule must be specified, see *INTEGRA-
TION_SHELL.  See remarks below. 
Remarks: 
Isotropic  hardening  for  both  materials  is  assumed.    The  material  to  which  the  glass  is 
bonded is assumed to stretch plastically without failure.  A user defined integration rule 
specifies  the  thickness  of  the  layers  making  up  the  glass.    Fi  defines  whether  the 
integration  point  is  glass  (0.0)  or  polymer  (1.0).    The  material  definition,  Fi,  has  to  be 
given  for  the  same  number  of  integration  points  (NIPTS)  as  specified  in  the  rule.    A 
maximum of 32 layers is allowed. 
If  the  recommended  user  defined  rule  is  not  defined,  the  default  integration  rules  are 
used.  The location of the integration points in the default rules are defined in the *SEC-
TION_SHELL keyword description.
*MAT_BARLAT_ANISOTROPIC_PLASTICITY 
This is Material Type 33.  This model was developed by Barlat, Lege, and Brem [1991] 
for  modeling  anisotropic  material  behavior  in  forming  processes.    The  finite  element 
implementation  of  this  model  is  described  in  detail  by  Chung  and  Shah  [1992]  and  is 
used  here.    It  is  based  on  a  six  parameter  model,  which  is  ideally  suited  for  3D 
continuum problems, see notes below.  For sheet forming problems, material 36 based 
on a 3-parameter model is recommended. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
Variable 
Type 
1 
A 
F 
  Card 3 
1 
2 
RO 
F 
2 
B 
F 
2 
Variable 
AOPT 
BETA 
Type 
F 
F 
  Card 4 
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
3 
E 
F 
3 
C 
F 
3 
3 
ZP 
F 
4 
PR 
F 
4 
F 
F 
4 
4 
A1 
F 
5 
K 
F 
5 
G 
F 
5 
5 
A2 
F 
6 
E0 
F 
6 
H 
F 
6 
6 
A3 
F 
7 
N 
F 
7 
LCID 
F 
7 
8 
M 
F 
8 
8 
7
Card 5 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
7 
8 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
E 
PR 
K 
EO 
N 
M 
A 
B 
C 
F 
G 
H 
LCID 
Mass density. 
Young’s modulus, 𝐸. 
Poisson’s ratio, 𝜈. 
𝑘, strength coefficient, see notes below. 
𝜀0, strain corresponding to the initial yield, see notes below. 
𝑛, hardening exponent for yield strength. 
𝑚, flow potential exponent  in Barlat’s Model. 
𝑎, anisotropy coefficient in Barlat’s Model. 
𝑏, anisotropy coefficient in Barlat’s Model. 
𝑐, anisotropy coefficient in Barlat’s Model. 
𝑓 , anisotropy coefficient in Barlat’s Model. 
𝑔, anisotropy coefficient in Barlat’s Model. 
ℎ, anisotropy coefficient in Barlat’s Model. 
Option  load  curve  ID  defining  effective  stress  versus  effective
plastic  strain.    If  nonzero,  this  curve  will  be  used  to  define  the
yield  stress.      The  load  curve  is  implemented  for  solid  elements
only.
*MAT_BARLAT_ANISOTROPIC_PLASTICITY 
DESCRIPTION
AOPT 
Material axes option: 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by 
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES, and then, for shells only, rotated about
the shell element normal by an angle BETA.. 
EQ.1.0: locally orthotropic with material axes determined by a
point  in  space  and  the  global  location  of  the  element
center, this is the 𝑎-direction. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by 
offsetting the material axes by an angle, BETA, from a
line determined by taking the cross product of the vec-
tor 𝐯 with the normal to the plane of the element. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR). 
BETA 
Material  angle  in  degrees  for  AOPT = 1  (shells  only)  and 
AOPT = 3,  may  be  overridden  on  the  element  card,  see  *ELE-
MENT_SHELL_BETA or *ELEMENT_SOLID_ORTHO. 
MACF 
Material axes change flag for brick elements: 
EQ.1: No change, default, 
EQ.2: switch material axes 𝑎 and 𝑏, 
EQ.3: switch material axes 𝑎 and 𝑐, 
EQ.4: switch material axes 𝑏 and 𝑐. 
XP, YP, ZP 
Coordinates of point 𝐩 for AOPT = 1. 
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3. 
D1, D2, D3 
Components of vector 𝐝 for AOPT = 2.
Remarks: 
The yield function Φ is defined as: 
Φ = |𝑆1 − 𝑆2|𝑚 + ∣𝑆2 − 𝑆3∣𝑚 + ∣𝑆3 − 𝑆1∣𝑚 = 2𝜎̅̅̅̅̅ 𝑚 
where  𝜎̅̅̅̅̅  is  the  effective  stress  and  𝑆𝑖=1,2,3  are  the  principal  values  of  the  symmetric 
matrix 𝑆𝛼𝛽, 
𝑆𝑥𝑥 = [𝑐(𝜎𝑥𝑥 − 𝜎𝑦𝑦) − 𝑏(𝜎𝑧𝑧 − 𝜎𝑥𝑥)] 3⁄  
𝑆𝑦𝑦 = [𝑎(𝜎𝑦𝑦 − 𝜎𝑧𝑧) − 𝑐(𝜎𝑥𝑥 − 𝜎𝑦𝑦)] 3⁄  
𝑆𝑧𝑧 = [𝑏(𝜎𝑧𝑧 − 𝜎𝑥𝑥) − 𝑎(𝜎𝑦𝑦 − 𝜎𝑧𝑧)] 3⁄  
𝑆𝑦𝑧 = 𝑓 𝜎𝑦𝑧 
𝑆𝑧𝑥 = 𝑔𝜎𝑧𝑥 
𝑆𝑥𝑦 = ℎ𝜎𝑥𝑦 
The material constants a, b, c, f, g and h represent anisotropic properties.  When 
𝑎 = 𝑏 = 𝑐 = 𝑓 = 𝑔 = ℎ = 1, 
the  material  is  isotropic  and  the  yield  surface  reduces  to  the  Tresca  yield  surface  for 
𝑚 = 1 and von Mises yield surface for 𝑚 = 2 or 4. 
For  face  centered  cubic  (FCC)  materials 𝑚 = 8  is  recommended  and  for body  centered 
cubic (BCC) materials 𝑚 = 6 is used.  The yield strength of the material is 
𝜎𝑦 = 𝑘(𝜀𝑝 + 𝜀0)𝑛 
where  𝜀0 is the strain corresponding to the initial yield stress and 𝜀𝑝 is the plastic strain.
*MAT_BARLAT_YLD96 
This  is  Material  Type  33.    This  model  was  developed  by  Barlat,  Maeda,  Chung, 
Yanagawa,  Brem,  Hayashida,  Lege,  Matsui,  Murtha,  Hattori,  Becker,  and  Makosey 
[1997] for modeling anisotropic material behavior in forming processes in particular for 
aluminum alloys.  This model is available for shell elements only. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
Variable 
1 
E0 
Type 
F 
  Card 3 
Variable 
1 
C1 
Type 
F 
  Card 4 
1 
2 
RO 
F 
2 
N 
F 
2 
C2 
F 
2 
3 
E 
F 
3 
ESR0 
F 
3 
C3 
F 
3 
4 
PR 
F 
4 
M 
F 
4 
C4 
F 
4 
5 
K 
F 
5 
HARD 
F 
5 
AX 
F 
5 
6 
7 
8 
6 
A 
F 
6 
AY 
F 
6 
7 
8 
7 
8 
AZ0 
AZ1 
F 
7 
F 
8 
Variable 
AOPT 
BETA 
Type 
F
1 
2 
3 
Variable 
Type 
  Card 6 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
*MAT_033_96 
7 
8 
7 
8 
6 
A3 
F 
6 
D3 
F 
4 
A1 
F 
4 
D1 
F 
5 
A2 
F 
5 
D2 
F 
DESCRIPTION
  VARIABLE   
MID 
RO 
E 
PR 
K 
EO 
N 
ESR0 
M 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus, 𝐸. 
Poisson’s ratio,𝜈. 
𝑘, strength coefficient or a in Voce, see notes below. 
𝜀0, strain corresponding to the initial yield or b in Voce, see notes 
below. 
𝑛, hardening exponent for yield strength or c in Voce. 
𝜀SR0, in powerlaw rate sensitivity. 
𝑚, exponent for strain rate effects 
HARD 
Hardening option: 
LT.0.0:  absolute value defines the load curve ID. 
EQ.1.0: powerlaw 
EQ.2.0: Voce 
A 
C1 
Flow potential exponent. 
𝑐1, see equations below.
VARIABLE   
DESCRIPTION
C2 
C3 
C4 
AX 
AY 
AZ0 
AZ1 
𝑐2, see equations below. 
𝑐3, see equations below. 
𝑐4, see equations below. 
𝑎𝑥, see equations below. 
𝑎𝑦, see equations below. 
𝑎𝑧0, see equations below. 
𝑎𝑧1, see equations below. 
AOPT 
Material axes option: 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES,  and  then  rotated  about  the  shell  ele-
ment normal by an angle BETA. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
offsetting the material axes by an angle, BETA, from a
line determined by taking the cross product of the vec-
tor 𝐯 with the normal to the plane of the element. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID 
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  
BETA 
Material angle in degrees for AOPT = 0 and 3, may be overridden 
on the element card, see *ELEMENT_SHELL_BETA.. 
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3. 
D1, D2, D3 
Components of vector 𝐝 for AOPT = 2.
*MAT_033_96 
The yield stress 𝜎𝑦 is defined three ways.  The first, the Swift equation, is given in terms 
of the input constants as: 
𝜎𝑦 = 𝑘(𝜀0 + 𝜀𝑝)𝑛 (
𝜀̇
𝜀𝑆𝑅0
)
The second, the Voce equation, is defined as: 
𝜎𝑦 = 𝑎 − 𝑏𝑒−𝑐𝜀𝑝
and the third option is to give a load curve ID that defines the yield stress as a function 
of effective plastic strain.  The yield function Φ is defined as: 
Φ = 𝛼1|𝑠1 − 𝑠2|𝑎 + 𝛼2∣𝑠2 − 𝑠3∣𝑎 + 𝛼3∣𝑠3 − 𝑠1∣𝑎 = 2𝜎𝑦
𝑎 
where  𝑠𝑖    is  a  principle  component  of  the  deviatoric  stress  tensor  where  in  vector 
notation: 
and 𝐋 is given as 
𝐬 = 𝐋𝛔 
𝐋 =  
𝑐2 + 𝑐3
−𝑐3
−𝑐2
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
−𝑐3
𝑐3 + 𝑐1
−𝑐1
3 
−𝑐2
−𝑐1
𝑐1 + 𝑐2
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
𝑐4⎦
A coordinate transformation relates the material frame to the principle directions of 𝐬 is 
used to obtain the 𝛼𝑘 coefficients consistent with the rotated principle axes: 
2 + 𝛼𝑦𝑝2𝑘
2  
2 + 𝛼𝑧𝑝3𝑘
𝛼𝑘 = 𝛼𝑥𝑝1𝑘
𝛼𝑧 = 𝛼𝑧0cos2(2𝛽) + 𝛼𝑧1sin2(2𝛽) 
where 𝑝𝑖𝑗 are components of the transformation matrix.  The angle 𝛽 defines a measure 
of  the  rotation  between  the  frame  of  the  principal  value  of  𝐬  and  the  principal 
anisotropy axes.
*MAT_FABRIC 
This  is  Material  Type  34.    This  material  is  especially  developed  for  airbag  materials.  
The fabric model is a variation on the layered orthotropic composite model of material 
22 and is valid for 3 and 4 node membrane elements only. 
In addition to being a constitutive model, this model also invokes a special membrane 
element  formulation  which  is  more  suited  to  the  deformation  experienced  by  fabrics 
under large deformation.  For thin fabrics, buckling can result in an inability to support 
compressive  stresses;  thus  a  flag  is  included  for  this  option.    A  linearly  elastic  liner  is 
also  included  which  can  be  used  to  reduce  the  tendency  for  these  elements  to  be 
crushed  when  the  no-compression  option  is  invoked.    In  LS-DYNA  versions  after  931 
the isotropic elastic option is available. 
2 
RO 
F 
2 
3 
EA 
F 
3 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
Variable 
GAB 
Type 
F 
Remarks 
  Card 3 
1 
2 
3 
4 
EB 
F 
4 
CSE 
F 
1 
4 
5 
6 
7 
8 
PRBA 
PRAB 
F 
6 
F 
7 
8 
PRL 
LRATIO 
DAMP 
F 
4 
6 
F 
4 
7 
F 
8 
5 
EL 
F 
4 
5 
Variable 
AOPT 
FLC/X2 
FAC/X3 
ELA 
LNRC 
FORM 
FVOPT 
TSRFAC 
Type 
F 
Remarks 
F 
2 
F 
2 
F 
3 
F 
4 
F 
11 
F 
9 
F 
10
BETA 
ISREFG 
F 
I 
8 
7 
RL 
F 
*MAT_FABRIC 
*MAT_034 
  Card 4 
1 
2 
3 
Variable 
RGBRTH 
A0REF 
Type 
F 
F 
  Card 5 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
A1 
F 
4 
5 
A2 
F 
5 
6 
A3 
F 
6 
7 
X0 
F 
7 
8 
X1 
F 
8 
Additional card for FORM = 4, 14, or -14. 
  Card 6 
1 
2 
3 
4 
5 
6 
Variable 
LCA 
LCB 
LCAB 
LCUA 
LCUB 
LCUAB 
Type 
I 
I 
I 
I 
I 
I 
Additional card for FORM = -14.  
  Card 7 
1 
2 
Variable 
LCAA 
LCBB 
Type 
I 
I 
3 
H 
F 
4 
DT 
F 
5 
6 
7 
8 
ECOAT 
SCOAT 
TCOAT 
F 
F 
F 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density.
VARIABLE   
DESCRIPTION
EA 
EB 
PRBA 
PRAB 
GAB 
Young’s  modulus  -  longitudinal  direction.    For  an  isotopic  elastic
fabric material only EA and PRBA are defined and are used as the
isotropic  Young’s  modulus  and  Poisson’s  ratio,  respectively.    The
input for the fiber directions and liner should be input as zero for
the isotropic elastic fabric 
Young’s  modulus  -  transverse  direction,  set  to  zero  for  isotropic
elastic material. 
𝜈𝑏𝑎, Minor Poisson’s ratio ba direction. 
𝜈𝑎𝑏, Major Poisson’s ratio ab direction.   
𝐺𝑎𝑏,  shear  modulus  ab  direction,  set  to  zero  for  isotropic  elastic
material. 
CSE 
Compressive stress elimination option : 
EL 
PRL 
LRATIO 
DAMP 
AOPT 
EQ.0.0: don’t eliminate compressive stresses, (default) 
EQ.1.0: eliminate  compressive  stresses.    This  option  does  not
apply to the liner. 
Young’s modulus for elastic liner (required if LRATIO > 0). 
Poisson’s ratio for elastic liner (required if LRATIO > 0). 
A non-zero value activates the elastic liner and defines the ratio of
liner thickness to total fabric thickness (optional). 
Rayleigh  damping  coefficient.    A  0.05  coefficient  is  recommended 
corresponding to 5% of critical damping.  Sometimes larger values
are necessary. 
Material  axes  option  .    Also,  please  refer  to  Remark  5  for 
additional information specific to fibre directions for fabrics: 
EQ.0.0:  locally  orthotropic  with  material  axes  determined  by
element  nodes  1,  2,  and  4,  as  with  *DEFINE_COORDI-
NATE_NODES,  and  then  rotated  about  the  element
normal by an angle BETA.  
EQ.2.0:  globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR.
*MAT_034 
DESCRIPTION
EQ.3.0:  locally orthotropic material axes determined by rotating
the material axes about the element normal by an angle,
BETA, from a line in the plane of the element defined by
the  cross  product  of  the  vector v  with  the  element  nor-
mal. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).    Available  in  R3  version  of  971 
and later. 
If X0 is between 0 and 1 (exclusive) then 
X2 (FLC) 
X3 (FAC) 
X2  is  a  coefficient  of  the  porosity  from  the  equation  in  Anagonye
and Wang [1999]. 
X3 is a coefficient of the porosity equation of Anagonye and Wang 
[1999]. 
Else If X0 = 0 or -1 then (sets meaning of the abscissa for load curve cases) 
FLC (X2) 
Optional porous leakage flow coefficient.   
GE.0:  Porous leakage flow coefficient. 
LT.0:  |FLC|  is  interpreted  as  a  load  curve  ID  defining  FLC  as  a 
function of time. 
If FVOPT < 7 then (sets meaning of the mantissa for load curve case) 
FAC (X3) 
Optional characteristic fabric parameter.   
GE.0: Characteristic fabric parameter 
LT.0:  |FAC| is interpreted as a load curve ID defining FAC as a
function of absolute pressure.
VARIABLE   
DESCRIPTION
Else if FVOPT ≥ 7 then (sets meaning of the mantissa for load curve case) 
FAC (X3) 
Optional characteristic fabric parameter.   
GE.0:  Characteristic fabric parameter 
LT.0:  |FAC| is  interpreted  as  a  load  curve  ID  giving  leakage 
volume  flux  rate  versus  absolute  pressure.    The  volume 
flux (per area) rate (per time) has the unit of 
𝑑(volflux) dt⁄ ≈ [length]3 ([length]2[time])
, 
≈ [length] [time]
⁄
⁄
equivalent to relative porous gas speed. 
End if 
Else if X0 = 1 (sets meaning of the abscissa for load curve cases) 
FLC (X2) 
Optional porous leakage flow coefficient.   
GE.0:  Porous leakage flow coefficient. 
LT.0:  |FLC| is interpreted as a load curve curve ID defining FLC
versus the stretching ratio defined as 𝑟𝑠 = 𝐴/𝐴0.  See notes 
below. 
If FVOPT  >  7 then (sets meaning of the mantissa for load curve case) 
FAC (X3) 
Optional characteristic fabric parameter.   
GE.0: Characteristic fabric parameter 
LT.0:  |FAC|  is  interpreted  as  a  load  curve  defining  FAC  versus
the pressure ratio 𝑟𝑝 = 𝑃ai𝑟/𝑃bag.  See Remark 2 below.
DESCRIPTION
*MAT_034 
Else if FVOPT ≥ 7 then (sets meaning of the mantissa for load curve case) 
FAC (X3) 
Optional characteristic fabric parameter.   
GE.0:  Characteristic fabric parameter 
LT.0:  |FAC|  is  interpreted  as  a  load  curve  defining  leakage 
volume 
flux  rate  versus  the  pressure  ratio  defined 
as 𝑟𝑝 = 𝑃air/𝑃bag.  See  Remark  2  below.    The  volume  flux 
(per area) rate (per time) has the unit of 
𝑑(volflux) dt⁄ ≈ [length]3 ([length]2[time])
, 
≈ [length] [time]
⁄
⁄
equivalent to relative porous gas speed. 
End if 
End if 
ELA 
Effective leakage area for blocked fabric, ELA : 
LT.0.0: |ELA|  is  the  load  curve  ID  of  the  curve  defining  ELA
versus  time.    The  default  value  of  zero  assumes  that  no
leakage occurs.  A value of .10 would assume that 10% of
the blocked fabric is leaking gas. 
LNRC 
Flag to turn off compression in liner until the reference geometry is
reached, i.e., the fabric element becomes tensile. 
EQ.0.0: off. 
EQ.1.0: on. 
FORM 
Flag to modify membrane formulation for fabric material: 
EQ.0.0:  default.  Least costly and very reliable. 
EQ.1.0: 
invariant local membrane coordinate system 
EQ.2.0:  Green-Lagrange strain formulation 
EQ.3.0: 
EQ.4.0: 
large  strain  with  nonorthogonal  material  angles.    See
Remark 5. 
large  strain  with  nonorthogonal  material  angles  and
nonlinear stress strain behavior.  Define optional load
curve IDs on optional card. 
EQ.12.0:  Enhanced version of formulation 2.  See Remark 11.
VARIABLE   
DESCRIPTION
EQ.13.0:  Enhanced version of formulation 3.  See Remark 11. 
EQ.14.0:  Enhanced version of formulation 4.  See Remark 11. 
EQ.-14.0:  Same as formulation 14, but invokes reading of card 7.
See Remark 14. 
EQ.24.0:  Enhanced version of formulation 14.  See Remark 11. 
FVOPT 
Fabric venting option. 
EQ.1: Wang-Nefske  formulas  for  venting  through  an  orifice  are 
used.  Blockage is not considered. 
EQ.2: Wang-Nefske  formulas  for  venting  through  an  orifice  are
used.    Blockage  of  venting  area  due  to  contact  is  consid-
ered. 
EQ.3: Leakage  formulas  of  Graefe,  Krummheuer,  and  Siejak
[1990] are used.  Blockage is not considered. 
EQ.4: Leakage  formulas  of  Graefe,  Krummheuer,  and  Siejak
[1990] are used.  Blockage of venting area due to contact is
considered. 
EQ.5: Leakage formulas based on flow through a porous media
are used.  Blockage is not considered. 
EQ.6: Leakage formulas based on flow through a porous media
are  used.    Blockage of  venting  area  due  to  contact  is  con-
sidered. 
EQ.7: Leakage  is  based  on  gas  volume  outflow  versus  pressure
load curve [Lian, 2000].  Blockage is not considered.  Abso-
lute  pressure  is  used  in  the  porous-velocity-versus-
pressure  load  curve,  given  as  FAC  in  the  *MAT_FABRIC 
card. 
EQ.8: Leakage  is  based  on  gas  volume  outflow  versus  pressure
load curve [Lian 2000].  Blockage of venting or porous area
due to contact is considered.  Absolute pressure is used in 
the  porous-velocity-versus-pressure  load  curve,  given  as 
FAC in the *MAT_FABRIC card.
DESCRIPTION
TSRFAC 
Strain restoration factor 
*MAT_034 
LT.0: 
|TSRFAC|  is  the  ID of  a  curve  defining  TSRFAC 
versus time.. 
GT.0 and LT.1:  TSRFAC applied from time 0. 
GE.1: 
TSRFAC  is  the  ID  of  a  curve  that  defines
TSRFAC  versus  time  using  an  alternate  method
(not available for FORM = 0 or 1). 
RGBRTH 
Material dependent birth time of airbag reference geometry.  Non-
zero RGBRTH overwrites the birth time defined in the *AIRBAG_-
REFERENCE_GEOMETRY_BIRTH section.   RGBRTH also applies 
to  reference  geometry  defined  by  *AIRBAG_SHELL_REFER-
ENCE_GEOMETRY. 
A0REF 
Calculation  option  of  initial  area,  A0,  used  for  airbag  porosity 
leakage calculation. 
EQ.0.:  default.  Use the initial geometry defined in *NODE. 
EQ.1.:  Use 
the 
reference 
geometry 
*AIRBAG_REFERENCE_GEOMETRY 
*AIRBAG_SHELL_REFERENCE_GEOMETRY. 
defined 
in
or
A1, A2, A3 
Components of vector a for AOPT = 2. 
X0, X1 
Coefficients  of  Anagonye  and  Wang  [1999]  porosity  equation  for
the leakage area: 𝐴leak = 𝐴0(𝑋0 + 𝑋1𝑟𝑠 + 𝑋2𝑟𝑝 + 𝑋3𝑟𝑠𝑟𝑝) 
X0.EQ.-1:  Compressing  seal  vent  option.    The  leakage  area  is
evaluated as 𝐴leak = max(𝐴current − 𝐴0, 0). 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3. 
BETA 
ISREFG 
Material angle in degrees for AOPT = 0 and 3, may be overridden 
on the element card, see *ELEMENT_SHELL_BETA. 
Initialize  stress  by  *AIRBAG_REFERENCE_GEOMETRY.    This 
option  applies  only  to  FORM = 12.    Note  that  *MAT_FABRIC 
cannot  be  initialized  using  a  dynain  file  because  *INITIAL_-
STRESS_SHELL is not applicable to *MAT_FABRIC. 
EQ.0.0: default.  Not active. 
EQ.1.0: active
LCA 
LCB 
LCAB 
LCUA 
LCUB 
LCUAB 
RL 
LCAA 
*MAT_FABRIC 
DESCRIPTION
Load  curve  or  table  ID.    Load  curve  ID  defines  the  stress  versus
uniaxial  strain  along  the  a-axis  fiber.    Table  ID  defines  for  each 
strain  rate  a  load  curve  representing  stress  versus  uniaxial  strain
along  the  a-axis  fiber.    Available  for  FORM = 4,  14,  –14,  and  24 
only,  table  allowed  only  for  form = -14.    If  zero,  EA  is  used.    For 
FORM = 14, -14, and 24, this curve can be defined in  both tension
and compression, see Remark 6 below. 
Load  curve  or  table  ID.    Load  curve  ID  defines  the  stress  versus 
uniaxial  strain  along  the  b-axis  fiber.    Table  ID  defines  for  each 
strain  rate  a  load  curve  representing  stress  versus  uniaxial  strain
along  the  b-axis  fiber.    Available  for  FORM = 4,  14,  -14,  and  24 
only,  table  allowed  only  for  form = -14.    If  zero,  EB  is  used.    For 
FORM = 14, -14, and 24, this curve can be defined in  both tension
and compression, see Remark 6 below. 
Load curve ID for shear stress versus shear strain in the ab-plane; 
available for FORM = 4, 14, -14, and 24 only.  If zero, GAB is used. 
Unload/reload  curve  ID  for  stress  versus  strain  along  the  a-axis 
fiber; available for FORM = 4, 14, -14, and 24 only.  If zero, LCA is 
used. 
Unload/reload  curve  ID  for  stress  versus  strain  along  the  b-axis 
fiber; available for FORM = 4, 14, -14, and 24 only.  If zero, LCB is 
used. 
Unload/reload curve ID for shear stress versus shear strain in the
ab-plane;  available  for  FORM = 4,  14,  -14,  and  24  only.    If  zero, 
LCAB is used. 
Optional  reloading  parameter  for  FORM = 14  and  24.    Values 
between  0.0  (reloading  on  unloading  curve-default)  and  1.0 
(reloading  on  a  minimum  linear  slope  between  unloading  curve
and loading curve) are possible. 
Load curve or table ID.  Load curve ID defines the stress along the
a-axis  fiber  versus  biaxial  strain.    Table  ID  defines  for  each
directional strain rate a load curve representing stress along the a-
axis  fiber  versus  biaxial  strain.    Available  for  FORM=–14  only,  if 
zero, LCA is used.
LCBB 
*MAT_034 
DESCRIPTION
Load curve or table ID.  Load curve ID defines the stress along the
b-axis  fiber  versus  biaxial  strain.    Table  ID  defines  for  each
directional strain rate a load curve representing stress along the b-
axis  fiber  versus  biaxial  strain.    Available  for  FORM=–14  only,  if 
zero, LCB is used. 
H 
DT 
Normalized hysteresis parameter between 0 and 1. 
Strain rate averaging option. 
EQ.0.0: Strain rate is evaluated using a running average. 
LT.0.0:  Strain  rate  is  evaluated  using  average  of  last  11  time 
steps. 
GT.0.0: Strain rate is averaged over the last DT time units. 
ECOAT 
Young’s modulus of coat material, see Remark 14. 
SCOAT 
Yield stress of coat material, see Remark 14. 
TCOAT 
Thickness  of  coat  material,  may  be  positive  or  negative,  see
Remark 14. 
Remarks: 
1.  The  Compressive  Stress  Elimination  Option  for  Airbag  Wrinkling.    Setting 
CSE=1  switches  off  compressive  stress  in  the  fabric,  thereby  eliminating  wrin-
kles.  Without this “no compression” option the geometry of the bag’s wrinkles 
control  the  amount  of  mesh  refinement.    In  eliminating  the  wrinkles,  this  fea-
ture reduces the number of elements needed to attain an accurate solution. 
The no compression option can allow elements to collapse to a line which can 
lead to elements becoming tangled.  The elastic liner option is one way to add 
some  stiffness  in  compression  to  prevent  this,  see  Remark  4.    Alternatively, 
when  using  fabric  formulations  14,  -14,  or  24    tangling  can  be  re-
duced  by  defining  stress/strain  curves  that  include  negative  strain  and  stress 
values.  See Remark 6.use 
2.  Porosity.  The parameters FLC and FAC are optional for the Wang-Nefske and 
Hybrid inflation models.  It is possible for the airbag to be constructed of multi-
ple  fabrics  having  different  values  for  porosity  and  permeability.    Typically,
FLC and FAC must be determined experimentally and their variations in time 
or with pressure are optional to allow for maximum flexibility. 
3.  Effects of Airbag-Structure Interaction on Porosity.  To calculate the leakage 
of  gas  through  the  fabric  it  is  necessary  to  accurately  determine  the  leakage 
area.  The dynamics of the airbag may cause the leakage area to change during 
the  course  of  the  simulation.    In  particular,  the  deformation  may  change  the 
leakage area, but the leakage area may also decrease when the contact between 
the airbag and the structure blocks the flow.  LS-DYNA can check the interac-
tion  of  the  bag  with  the  structure  and  split  the  areas  into  regions  that  are 
blocked and unblocked depending on whether the regions are in or not in con-
tact, respectively.  Blockage effects may be controlled with the ELA field. 
4.  Elastic  Liner.    An  optional  elastic  liner  can  be  defined  using  EL,  PRL  and 
LRATIO.  The liner is an isotropic layer that acts in both tension and compres-
sion.  However, setting, LNRC to 1.0 eliminates compressive stress in the liner 
until  both  principle  stresses  are  tensile.    The  compressive  stress  elimination 
option, CSE=1, has no influence on the liner behavior. 
5.  Fiber Axes.  For formulations 0, 1, and 2,  the 𝑎-axis and 𝑏-axis fiber 
directions are assumed to be orthogonal and are completely defined by the materi-
al axes option, AOPT=0, 2, or 3.  For FORM=3, 4, 13, or 14, the fiber directions 
are not assumed orthogonal and must be specified using the ICOMP=1 option on 
*SECTION_SHELL.    Offset  angles  should  be  input  into  the  B1  and  B2  fields 
used  normally  for  integration  points  1  and  2.    The  𝑎-axis  and  𝑏-axis  directions 
will then be offset from the 𝑎-axis direction as determined by the material axis 
option, AOPT=0, 2, or 3. 
6.  Stress vs.  Strain Curves.  For formulations  4, 14, -14, and 24, 2nd 
Piola-Kirchhoff  stress  vs.    Green’s  strain  curves  may  be  defined  for  𝑎-axis,  𝑏-
axis, and shear stresses for loading and also for unloading and reloading.  Al-
ternatively,  the  𝑎-axis  and  𝑏-axis  curves  can  be  input  using  engineering  stress 
vs.  strain by setting DATYP = -2 on *DEFINE_CURVE. 
Additionally, for formulations 14, -14, and 24, the uniaxial loading curves LCA 
and LCB may be defined for negative values of strain and stress, i.e., a straight-
forward extension of the curves into the compressive region.  This is available 
in  order  to  model  the  compressive  stresses  resulting  from  tight  folding  of  air-
bags. 
The 𝑎-axis and 𝑏-axis stress follow the curves for the entire defined strain region 
and if compressive behavior is desired the user should preferably make sure the 
curve  covers  all  strains  of  interest.    For  strains  below  the  first  point  on  the 
curve, the curve is extrapolated using the stiffness from the constant values, EA 
or EB.
Shear  stress/strain  behavior  is  assumed  symmetric  and  curves  should  be  de-
fined for positive strain only.  However, formulations 14, -14, and 24 allow the 
extending  of the  curves  in  the  negative  strain  region to  model  asymmetric  be-
havior.    The  asymmetric  option  cannot  be  used  with  a  shear  stress  unload 
curve.  If a load curve is omitted, the stress  is calculated from the  appropriate 
constant modulus, EA, EB, or GAB. 
7.  Yield  Behavior.    When  formulations  4,  14,  -14,  and  24    are  used 
with  loading  and  unloading  curves  the  initial  yield  strain  is  set  equal  to  the 
strain  of  the  first  point  in  the  load  curve  having  a  stress  greater  than  zero.  
When  the  current  strain  exceeds  the  yield  strain,  the  stress  follows  the  load 
curve  and  the  yield  strain  is  updated  to  the  current  strain.    When  unloading 
occurs, the unload/reload curve is shifted along the x-axis until it intersects the 
load curve at the current yield strain.  When using unloading curves, compres-
sive  stress  elimination  should  be  active  to  prevent  the  fibers  from  developing 
compressive  stress  during  unloading  when  the  strain  remains  tensile.    To  use 
this  option,  the  unload  curve  should  have  a  nonnegative  second  derivate  so  that  the 
curve will shift right as the yield stress increases. 
If  LCUA,  LCUB,  or  LCUAB  are  input  with  negative  values,  then  unloading  is 
handled  differently.    Instead  of  shifting  the  unload  curve  along  the 𝑥-axis,  the 
curve is stretched in both the 𝑥-direction and 𝑦-direction such that the first point 
remains  anchored  at  (0,0)  and  the  initial  intersection  point  of  the  curves  is 
moved  to  the  current  yield  point.    This  option  guarantees  the  stress  remains 
tensile while the strain is tensile so compressive stress elimination is not neces-
sary.  To use this option the unload curve should have an initial slope less steep than 
the load curve, and should steepen such that it intersects the load curve at some positive 
strain value. 
8.  Shear  Unload-Reload,  Fabric  Formulation,  and  LS-DYNA  version.    With 
release  6.0.0  of  version  971,  LS-DYNA  changed  the  way  that  unload/reload 
curves for shear stress-strain relations are interpreted.  Let f be the shear stress 
unload-reload curve LCUAB.  Then, 
where  the  scale  factors  𝑐1  and  𝑐2  depend  on  the  fabric  form    and 
version of LS-DYNA. 
𝜎𝑎𝑏 = 𝑐2𝑓 (𝑐1𝜀𝑎𝑏)
Fabric form 
4 
14 and -14 
24 
LS971 R5.1.0 and earlier 
LS971 R6.0.0 to R7.0 
LS-DYNA R7.1 and later 
𝑐1
2 
2 
2 
𝑐2
1 
1 
1 
𝑐1
2 
1 
1 
𝑐2
1 
2 
2 
𝑐1 
𝑐2 
- 
- 
1 
- 
- 
1 
When switching fabric forms or versions, the curve scale factors SFA and SFO 
on *DEFINE_CURVE can be used to offset this behavior. 
9.  Per Material Venting Option.  The FVOPT flag allows an airbag fabric venting 
equation to be assigned to a material.  The anticipated use for this option is to 
allow a vent to be defined using FVOPT=1 or 2 for one material and fabric leak-
age to be defined for using FVOPT=3, 4, 5, or 6 for other materials.  In order to 
use FVOPT, a venting option must first be defined for the airbag using the OPT 
parameter  on  *AIRBAG_WANG_NEFSKE  or  *AIRBAG_HYBRID.    If  OPT=0, 
then FVOPT is ignored.  If OPT is defined and FVOPT is omitted, then FVOPT 
is set equal to OPT. 
10.  TSRFAC  option  to  restore  element  strains.    Airbags  that  use  a  reference 
geometry will typically have nonzero strains at the start of the calculation.  To 
prevent  such  initial  strains  from  prematurely  opening  an  airbag,  initial  strains 
are stored and subtracted from the measured strain throughout the calculation. 
𝝈 = 𝑓 (𝜺 − 𝜺initial) 
•  Fabric formulations 2, 3, and 4  subtract off only the initial ten-
sile strains so these forms are typically used with CSE = 1 and LNRC = 1. 
•  Fabric  formulations  12,  13,  14,  -14,  and  24  subtract  off  the  total  initial 
strains so these forms may be used with CSE = 0 or 1 and LNRC = 0 or 1.  
A side effect of this strain modification is that airbags may not achieve the 
correct volume when they open.  Therefore, the TSRFAC option is imple-
mented to reduce the stored initial strain values over time thereby restor-
ing the total stain which drives the airbag towards the correct volume. 
During  each  cycle,  the  stored  initial  strains  are  scaled  by  (1.0 − TSRFAC).    A 
small value on the order of 0.0001 is typically sufficient to restore the strains in 
a few milliseconds of simulation time. 
The adjustment to restore initial strain is then, 
𝝈 = 𝑓 (𝜺 − 𝜺adjustment)
𝛆adjustment = εinitial ∏[1 − TSFRAC]
. 
a)  Time Dependent TSRFAC.  When TSRFAC ˂ 0, |TSRFAC| becomes the ID of 
a curve that defines TSRFAC as a function of time.  To delay the effect of 
TSRFAC,  the  curve  ordinate  value  should  be  initially  zero  and  should 
ramp  up  to  a  small  number  to  restore  the  strain  at  an  appropriate  time 
during the simulation.  The adjustment to restore initial strain is then, 
𝛆adjustment(𝑡𝑖) = εinitial ∏[1 − TSFRAC(𝑡𝑖)]
. 
To prevent airbags from opening prematurely, it is recommended to use 
the load curve option of TSRFAC to delay the strain restoration until the 
airbag is partially opened due to pressure loading. 
b)  Alternate Time Dependent TSRFAC.  For fabric formulations 2 and higher, a 
second  curve  option  is  invoked  by  setting  TSRFAC≥1  where  TSRFAC  is 
again  the  ID  of  a  curve  that  defines  TSRFAC  versus  time.    Like  the  first 
curve option, the stored initial strain values are scaled by (1.0 − TSRFAC), 
but the modified initial strains are not saved, so the effect of TSRFAC does 
not accumulate.  In this case the adjustment to eliminate initial strain  
𝛆adjustment(𝑡𝑖) = [1 − TSFRAC(𝑡𝑖)]𝛆initial. 
Therefore, the curve should ramp up from zero to one to fully restore the 
strain.    This  option  gives  the  user  better  control  of  the  rate  of  restoring 
the strain as it is a function of time rather than solution time step. 
11.  Enhancements  to  the  Material  Formulations.    Material  formulations   12, 13, and 14 are enhanced versions of formulations 2, 3, and 4, respec-
tively.  The most notable difference in their behavior is apparent when a refer-
ence  geometry  is  used  for the  fabric.    As  discussed  in  Remark 10, the  strain  is 
modified  to  prevent  initial  strains  from  prematurely  opening  an  airbag  at  the 
start of a calculation. 
Formulations 2, 3, and 4 subtract the initial tensile strains, while the enhanced 
formulations subtract the total initial strains.  Therefore, the enhanced formula-
tions  can  be  used  without  setting  CSE = 1  and  LNRC = 1  since  compressive 
stress cutoff is not needed to prevent initial airbag movement.  Formulations 2, 
3, and 4 need compressive stress cutoff when used with a reference geometry or 
they can generate compressive stress at the start of a calculation.  Available for 
formulation 12 only, the ISREFG parameter activates an option to calculate the 
initial stress by using a reference geometry. 
Material formulation 24 is an enhanced version of formulation 14 implementing 
a correction for Poisson’s effects when stress vs.  strain curves are input for the 
𝑎-fiber or 𝑏-fiber.  Also, for formulation 24, the outputted stress and strain in the
S 
A2
A1
loading 
unloading 
reloading 
E 
Figure M34-1. 
elout or d3plot database files is engineering stress and strain rather than the 2nd 
Piola Kirchoff and Green’s strain used by formulations other than 0 and 1. 
12.  Noise  Reduction  for  the  Strain  Rate  Measure.    If  tables  are  used,  then  the 
strain  rate  measure  is  the  time  derivative  of  the  Green-Lagrange  strain  in  the 
direction of interest.  To suppress noise, the strain rate is averaged according to 
the  value  of  DT.    If  DT > 0,  it  is  recommended  to  use  a  large  enough  value  to 
suppress the noise, while being small enough to not lose important information 
in the signal. 
13.  Hysteresis.    The  hysteresis  parameter  H  defines  the  fraction  of  dissipated 
energy during a load cycle in terms of the maximum possible dissipated ener-
gy.  Referring to the Figure M34-1, 
𝐻 ≈
𝐴1
𝐴1 + 𝐴2
14.  Coating  Feature  for  Additional  Rotational  Resistance.    It  is  possible  to 
model coating of the fabric using a sheet of elastic-ideal-plastic material where
the Young’s modulus, yield stress and thickness is specified for the coat materi-
al.  This will add rotational resistance to the fabric for a more realistic behavior 
of coated fabrics.  To read this parameters set FORM=-14, which adds an extra 
card  containing  the  three  parameters  ECOAT,  SCOAT  and  TCOAT,  corre-
sponding to the three coat material properties mentioned above. 
The thickness, TCOAT, applies to both sides of the fabric.  The coat material for 
a certain fabric element deforms along with this and all elements connected to 
this  element,  which  is  how  the  rotations  are  "captured".    Note  that  unless 
TCOAT  is  set  to  a  negative  value,  the  coating  will  add  to  the  membrane  stiff-
ness.    For  negative  values  of  TCOAT  the  thickness  is  set  to  |TCOAT|  and  the 
membrane  contribution  from  the  coating  is  suppressed.    For  this  feature  to 
work, the fabric parts must not include any  T-intersections, and all of the sur-
face normal vectors of connected fabric elements must point in the same direc-
tion.  This option increases the computational complexity of this material. 
15 
Fabric  forms  12,  13,  14,  -14,  and  24  allow  input  of  both  the  minor  Poisson’s 
ratio, 𝜈𝑏𝑎, and the major Poisson’s ratio, 𝜈𝑎𝑏.  This allows asymmetric Poisson’s 
behavior  to  be  modelled.    If  the  major  Poisson’s  ratio  is  left  blank  or  input  as 
zero, then it will be calculated using 𝜈𝑎𝑏 = 𝜈𝑏𝑎
.
𝐸𝑎
𝐸𝑏
*MAT_FABRIC_MAP 
This is Material Type 34 in which the stress response is given exclusively by tables, or 
maps,  and  where  some  obsolete  features  in  *MAT_FABRIC  have  been  deliberately 
excluded to allow for a clean input and better overview of the model. 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
4 
5 
6 
PXX 
PYY 
SXY 
DAMP 
Type 
A8 
F 
F 
  Card 2 
1 
Variable 
FVOPT 
Type 
F 
  Card 3 
1 
2 
X0 
F 
2 
3 
X1 
F 
3 
F 
4 
F 
5 
F 
6 
FLC/X2 
FAC/X3 
ELA 
F 
4 
F 
5 
F 
6 
7 
TH 
F 
7 
7 
Variable 
ISREFG 
CSE 
SRFAC 
BULKC 
JACC 
FXX 
FYY 
Type 
F 
  Card 4 
1 
F 
2 
F 
3 
F 
4 
Variable 
AOPT 
ECOAT 
SCOAT 
TCOAT 
Type 
F 
F 
F 
F 
  Card 5 
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
3 
ZP 
F 
4 
A1 
F 
F 
5 
5 
A2 
F 
F 
6 
6 
A3 
F 
F 
7 
7 
8 
2-246 (EOS) 
LS-DYNA R10.0 
8 
8 
8 
DT
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
  VARIABLE   
DESCRIPTION
*MAT_034M 
7 
8 
BETA 
F 
MID 
RO 
PXX 
PYY 
SXY 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Table giving engineering local 𝑋𝑋-stress as function of engineering 
local 𝑋𝑋-strain and 𝑌𝑌-strain. 
Table giving engineering local 𝑌𝑌-stress as function of engineering 
local 𝑌𝑌-strain and 𝑋𝑋-strain. 
Curve giving local 2nd Piola-Kirchhoff XY-stress as function of local 
Green 𝑋𝑌-strain. 
DAMP 
Damping coefficient for numerical stability. 
TH 
Table giving hysteresis factor 0 ≤ 𝐻 < 1 as function of engineering 
local 𝑋𝑋-strain and 𝑌𝑌-strain.  
GT.0.0: TH is table ID 
LE.0.0:  -TH is used as constant value for hysteresis factor 
FVOPT 
Fabric venting option, see *MAT_FABRIC. 
X0, X1 
Fabric venting option parameters, see *MAT_FABRIC. 
FLC/X2 
Fabric venting option parameter, see *MAT_FABRIC. 
FAC/X3 
Fabric venting option parameter, see *MAT_FABRIC. 
ELA 
Fabric venting option parameter, see *MAT_FABRIC. 
ISREFG 
Initial stress by reference geometry. 
EQ.0.0: Not active. 
EQ.1.0: Active
VARIABLE   
DESCRIPTION
CSE 
Compressive stress elimination option. 
EQ.0.0: Don’t eliminate compressive stresses, 
EQ.1.0: Eliminate compressive stresses. 
SRFAC 
Load  curve  ID  for  smooth  stress  initialization  when  using  a
reference geometry. 
BULKC 
Bulk modulus for fabric compaction. 
JACC 
FXX 
FYY 
Jacobian for the onset of fabric compaction. 
Load  curve  giving  scale  factor  of  uniaxial  stress  in  first  material
direction as function of engineering strain rate. 
Load curve giving scale factor of uniaxial stress in second material 
direction as function of engineering strain rate. 
DT 
Time window for smoothing strain rates used for FXX and FYY. 
AOPT 
Material axes option, see *MAT_FABRIC. 
ECOAT 
Young’s  modulus  of  coat  material  to  include  bending  properties. 
This  together  with  the  following  two  parameters  (SCOAT  and
TCOAT)  encompass  the  same  coating/bending  feature  as  in
*MAT_FABRIC.  Please refer to these manual pages and associated
remarks. 
SCOAT 
Yield stress of coat material, see *MAT_FABRIC. 
TCOAT 
Thickness  of  coat  material,  may  be  positive  or  negative,  see
*MAT_FABRIC. 
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3. 
D1, D2, D3 
Components of vector 𝐝 for AOPT = 2. 
BETA 
Material angle in degrees for AOPT = 0 and 3, may be overridden 
on the element card, see *ELEMENT_SHELL_BETA.
*MAT_034M 
This material model invokes a special membrane element formulation regardless of the 
element  choice.    It  is  an  anisotropic  hyperelastic  model  where  the  2nd  Piola-Kirchhoff 
stress  𝐒  is  a  function  of  the  Green-Lagrange  strain  𝐄  and  possibly  its  history.    Due  to 
anisotropy, this strain is transformed to obtain the strains in each of the fiber directions  
𝐸𝑋𝑋 and 𝐸𝑌𝑌 together with the shear strain 𝐸𝑋𝑌.  The associated stress components in 
the local system are given as functions of the strain components 
𝑆𝑋𝑋 = γ𝑆𝑋𝑋(𝐸𝑋𝑋, 𝐸𝑌𝑌)ϑ 
𝑆𝑌𝑌 = γ𝑆𝑌𝑌(𝐸𝑌𝑌, 𝐸𝑋𝑋)ϑ 
𝑆𝑋𝑌 = γ𝑆𝑋𝑌(𝐸𝑋𝑌)ϑ. 
The  factor  𝛾  is  used  for  dissipative  effects  and  is  described  in  more  detail  later,  for 
TH = 0,  𝛾 = 1,  and  the  function  ϑ  represents  a  strain  rate  scale  factor  also  described 
below,  for  FXX = FYY = 0  this  factor  is  1.  While  the  shear  relation  is  given  directly 
through the curve SXY, the tabular input of the fiber stress components PXX and PYY is 
for the sake of convenience the engineering stress as function of engineering strain, i.e., 
𝑃𝑋𝑋 = 𝑃𝑋𝑋(𝑒𝑋𝑋, 𝑒𝑌𝑌) 
𝑃𝑌𝑌 = 𝑃𝑌𝑌(𝑒𝑌𝑌, 𝑒𝑋𝑋). 
To this end, the following conversion formulae are used between stresses and strains 
𝑒 = √1 + 2𝐸 − 1 
𝑆 =
1 + 𝑒
these being applied in each of the two fiber directions. 
Compressive  stress  elimination  is  optional  through  the  CSE  parameter,  and  when 
activated  the  principal  components  of  the  2nd  Piola-Kirchhoff  stress  is  restricted  to 
positive values.  
If a reference geometry is used, then SRFAC is the identity of a curve that is a function 
𝛼(𝑡) that should increase from zero to unity during a short time span, during which the 
Green-Lagrange strain used in the formulae above is substituted for  
𝐄̃ = 𝐄 − [1 − 𝛼(𝑡)]𝐄0, 
where 𝑬0 is the strain at time zero.  This is done in order to smoothly initialize the stress 
resulting from using a reference geometry different from the geometry at time zero. 
The factor 𝛾 is a function of the strain history and is initially set to unity, and depends, 
more specifically, on the internal work 𝜖 given by the stress power 
𝜖 ̇ = 𝐒 ∶ 𝐄̇.
Figure M34M-1.  Cyclic loading model for hysteresis model H 
The  evolution  of  𝛾  is  related  to  the  stress  power  in  the  sense  that  it  will  increase  on 
loading  and  decrease  on  unloading,  and  in  this  way  introduce  dissipation.    The  exact 
mathematical formula is too complicated to reveal, but in essence the function looks like 
𝛾 = {
1 − 𝐻(𝑒 ̅𝑋𝑋, 𝑒𝑌𝑌) + 𝐻(𝑒 ̅𝑋𝑋, 𝑒𝑌𝑌)exp[𝛽(𝜖 − 𝜖)]
1 − 𝐻(𝑒 ̅𝑋𝑋, 𝑒𝑌𝑌)exp[−𝛽(𝜖 − 𝜖)]
𝜖 ̇ < 0
𝜖 ̇ ≥ 0
Here 𝜖 is the maximum attained internal work up to this point in time, 𝑒 ̅𝑋𝑋 and 𝑒 ̅𝑌𝑌 are 
the engineering strain values associated with value. 𝐻(𝑒 ̅𝑋𝑋, 𝑒𝑌𝑌) is the hysteresis factor 
defined by the user through the input parameter TH, it may or may not depend on the 
strains.  𝛽  is  a  decay  constant  that  depends  on  𝑒 ̅𝑋𝑋  and  𝑒 ̅𝑌𝑌,  and  𝜖  is  the  minimum 
attained  internal  work  at  any  point  in  time  after  𝜖  was  attained.    In  other  words,  on 
unloading  𝛾  will  exponentially  decay  to  1 − 𝐻  and  on  loading  it  will  exponentially 
grow to 1 and always be restricted by the lower and upper bounds, 1 − 𝐻 < 𝛾 ≤ 1.  The 
only thing the user needs to care about is to input a proper hysteresis factor 𝐻, and with 
reference to a general loading/unloading cycle illustrated in figure M34M-1 below the 
relation 1 − 𝐻 = 𝜖𝑢/𝜖𝑙 should hold. 
To account for the packing of yarns in compression, a compaction effect is modeled by 
adding a term to the strain energy function on the form 
𝑊𝑐 = 𝐾𝑐𝐽 {𝑙𝑛 (
𝐽𝑐
) − 1} ,  for 𝐽 ≤ 𝐽𝑐 
where  𝐾𝑐  (BULKC)  is  a  physical  bulk  modulus,  𝐽 = det(𝑭)  is  the  jacobian  of  the 
deformation and 𝐽𝑐 (JACC) is the critical jacobian for when the effect commences.  Here 
𝐅 is the deformation gradient.  This gives a contribution to the pressure given by 
𝑝 = 𝐾𝑐𝑙𝑛 (
𝐽𝑐
) ,  for 𝐽 ≤ 𝐽𝑐 
and thus prevents membrane elements from collapsing or inverting when subjected to 
compressive  loads.    The  bulk  modulus  𝐾𝑐  should  be  selected  with  the  slopes  in  the 
stress map tables in mind, presumably some order of magnitude(s) smaller.   
As an option, the local membrane stress can be scaled based on the engineering strain 
rates via the function 𝜗 = 𝜗(𝑒 ̇, 𝐒). We set
𝑒 ̇ = max (
𝜖 ̇
‖𝐅𝐒‖
, 0) 
to be the equivalent engineering strain rate in the direction of loading and define 
𝜗(𝑒 ̇, 𝑺) =
𝐹𝑋𝑋(𝑒 ̇)|𝑆𝑋𝑋| + 𝐹𝑌𝑌(𝑒 ̇)|𝑆𝑌𝑌| + 2|𝑆𝑋𝑌|
|𝑆𝑋𝑋| + |𝑆𝑌𝑌| + 2|𝑆𝑋𝑌|
, 
meaning that the strain rate scale factor defaults to the user input data FXX and FYY for 
uniaxial loading in the two material directions, respectively. Note that we only consider 
strain rate scaling in loading and not in unloading, and furthermore that the strain rates 
used  in  evaluating  the  curves  are  pre-filtered  using  the  time  window  DT  to  avoid 
excessive  numerical  noise.    To  this  end,  it  is  recommended  to  set  DT  to  a  time 
corresponding to at least hundred time steps or so.
*MAT_PLASTIC_GREEN-NAGHDI_RATE 
This is Material Type 35.  This model is available only for brick elements and is similar 
to model 3, but uses the Green-Naghdi Rate formulation rather than the Jaumann rate 
for the stress update.  For some cases this might be helpful.  This model also has a strain 
rate dependency following the Cowper-Symonds model. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
E 
F 
3 
4 
PR 
F 
4 
5 
6 
7 
8 
5 
6 
7 
8 
Variable 
SIGY 
ETAN 
SRC 
SRP 
BETA 
Type 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
SIGY 
ETAN 
SRC 
SRP 
BETA 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Density 
Young’s modulus 
Poisson’s ratio 
Yield stress 
Plastic hardening modulus 
Strain rate parameter, C 
Strain rate parameter, P 
Hardening parameter, 0 < β′ < 1
*MAT_3-PARAMETER_BARLAT_{OPTION} 
This  is  Material  Type  36.    This  model  was  developed  by  Barlat  and  Lian  [1989]  for 
modeling sheets with anisotropic materials under plane stress conditions.  This material 
allows  the  use  of  the  Lankford  parameters  for  the  definition  of  the  anisotropy.    This 
particular  development  is  due  to  Barlat  and  Lian  [1989].    A  version  of  this  material 
model  which  has  a  flow  limit  diagram  failure  option  is  *MAT_FLD_3-PARAME-
TER_BARLAT. 
Available options include: 
<BLANK> 
NLP 
The NLP option estimates failure using the Formability Index (F.I.), which accounts for 
the non-linear strain paths seen in metal forming applications .  The 
NLP  field  in  card  3  must  be  defined  when  using  this  option.    The  NLP  option  is  also 
available in *MAT_037, *MAT_125 and *MAT_226. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
Variable 
Type 
1 
M 
F 
2 
RO 
F 
2 
3 
E 
F 
3 
4 
PR 
F 
4 
5 
HR 
F 
5 
R00/AB 
R45/CB 
R90/HB 
LCID 
F 
F 
F 
I 
6 
P1 
F 
6 
E0 
F 
7 
P2 
F 
7 
SPI 
F 
8 
ITER 
F 
8 
P3 
F 
Define the following card if and only if M < 0 
Card opt. 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CRC1 
CRA1 
CRC2 
CRA2 
CRC3 
CRA3 
CRC4 
CRA4 
Type 
F 
F 
F 
F 
F 
F 
F
1 
Variable 
AOPT 
Type 
F 
  Card 4 
1 
Variable 
Type 
  Card 5 
Variable 
1 
V1 
Type 
F 
Optional card. 
2 
C 
F 
2 
2 
V2 
F 
3 
P 
F 
3 
3 
V3 
F 
*MAT_3-PARAMETER_BARLAT 
4 
5 
6 
7 
8 
VLCID 
PB 
NLP/HTA 
HTB 
F 
I/F 
I 
4 
A1 
F 
4 
D1 
F 
F 
8 
7 
HTC 
HTD 
F 
7 
F 
8 
BETA 
HTFLAG 
F 
F 
5 
A2 
F 
5 
D2 
F 
6 
A3 
F 
6 
D3 
F 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
USRFAIL 
LCBI 
LCSH 
Type 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus, 𝐸 
GT.0.0: Constant value, 
LT.0.0:  Load  curve  ID = (-E)  which  defines  Young’s  Modulus 
as a function of plastic strain.  See Remarks.
VARIABLE   
DESCRIPTION
PR 
HR 
Poisson’s ratio, ν 
Hardening rule: 
EQ.1.0: linear (default), 
EQ.2.0: exponential (Swift) 
EQ.3.0: load curve or table with strain rate effects 
EQ.4.0: exponential (Voce) 
EQ.5.0: exponential (Gosh) 
EQ.6.0: exponential (Hocket-Sherby) 
EQ.7.0: load curves in three directions 
EQ.8.0: table with temperature dependence 
EQ.9.0: 3d table with temperature and strain rate dependence 
P1 
Material parameter: 
HR.EQ.1.0: Tangent modulus, 
HR.EQ.2.0: 𝑘,  strength  coefficient  for  Swift  exponential  hard-
ening 
HR.EQ.4.0: 𝑎, coefficient for Voce exponential hardening 
HR.EQ.5.0: 𝑘,  strength  coefficient  for  Gosh  exponential  hard-
ening 
HR.EQ.6.0: 𝑎,  coefficient  for  Hocket-Sherby  exponential  hard-
ening 
HR.EQ.7.0:  load curve ID for hardening in 45 degree direction.
See Remarks. 
P2 
Material parameter: 
HR.EQ.1.0: Yield stress 
HR.EQ.2.0: 𝑛, exponent for Swift exponential hardening 
HR.EQ.4.0: 𝑐, coefficient for Voce exponential hardening 
HR.EQ.5.0: 𝑛, exponent for Gosh exponential hardening 
HR.EQ.6.0: 𝑐,  coefficient  for  Hocket-Sherby  exponential  hard-
ening 
HR.EQ.7.0:  load curve ID for hardening in 90 degree direction. 
See Remarks.
*MAT_3-PARAMETER_BARLAT 
DESCRIPTION
ITER 
Iteration flag for speed: 
ITER.EQ.0.0:  fully iterative 
ITER.EQ.1.0:  fixed at three iterations 
M 
CRCn 
CRAn 
R00 
Generally,  ITER = 0  is  recommended.    However,  ITER = 1  is 
somewhat  faster  and  may  give  acceptable  results  in  most 
problems. 
𝑚,  exponent  in  Barlat’s  yield  surface,  absolute  value  is  used  if
negative. 
Chaboche-Rousselier hardening parameters, see Remarks. 
Chaboche-Rousselier hardening parameters, see Remarks. 
𝑅00, Lankford parameter in 0 degree direction 
GT.0.0: Constant value, 
LT.0.0:  Load curve or Table ID = (-R00) which defines 𝑅 value 
as a function of plastic strain (Curve) or as a function of
temperature and plastic strain (Table).  See Remarks. 
R45 
𝑅45, Lankford parameter in 45 degree direction 
GT.0.0: Constant value, 
LT.0.0:  Load curve or Table ID = (-R45) which defines R value 
as a function of plastic strain (Curve) or as a function of 
temperature and plastic strain (Table).  See Remarks. 
R90 
𝑅90, Lankford parameter in 90 degree direction 
GT.0.0: Constant value, 
LT.0.0:  Load curve or Table ID = (-R90) which defines R value 
as a function of plastic strain (Curve) or as a function of 
temperature and plastic strain (Table).  See Remarks. 
AB 
CB 
HB 
LCID 
𝑎, Barlat89 parameter, which is read instead of R00 if PB > 0. 
𝑐, Barlat89 parameter, which is read instead of R45 if PB > 0. 
ℎ, Barlat89 parameter, which is read instead of R90 if PB > 0. 
Load curve/table ID for hardening in the 0 degree direction.  See
Remarks.
VARIABLE   
DESCRIPTION
E0 
Material parameter 
HR.EQ.2.0: 𝜀0  for  determining  initial  yield  stress  for  Swift
exponential hardening.  (Default = 0.0) 
HR.EQ.4.0: 𝑏, coefficient for Voce exponential hardening 
HR.EQ.5.0: 𝜀0  for  determining  initial  yield  stress  for  Gosh
exponential hardening.  (Default = 0.0) 
HR.EQ.6.0: 𝑏,  coefficient  for  Hocket-Sherby  exponential  hard-
ening 
SPI 
Case I:  if 𝜀0 is zero above and HR.EQ.2.0. (Default = 0.0) 
[1
⁄
]
(𝑛−1)
EQ.0.0:  𝜀0 = (𝐸
𝑘)
LE.0.02:  𝜀0 = SPI 
GT.0.02: 𝜀0 = (SPI
𝑘 )
[1
𝑛⁄ ]
Case II:  If HR.EQ.5.0 
The strain at plastic yield is determined by an iterative procedure 
based on the same principles as for HR.EQ.2.0. 
P3 
Material parameter: 
HR.EQ.5.0: 𝑝, parameter for Gosh exponential hardening 
HR.EQ.6.0: 𝑛, 
exponent 
for  Hocket-Sherby 
exponential 
hardening 
AOPT 
Material axes option : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES,  and  then  rotated  about  the  shell  ele-
ment normal by an angle BETA. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element 
defined  by  the  cross  product  of  the  vector  v  with  the
element normal.
C 
P 
VLCID 
PB 
NLP 
HTA 
HTB 
*MAT_3-PARAMETER_BARLAT 
DESCRIPTION
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).    Available  with  the  R3  release 
of Version 971 and later. 
𝐶 in Cowper-Symonds strain rate model 
𝑝 in Cowper-Symonds strain rate model, 𝑝 = 0.0 for no strain rate 
effects 
Volume correction curve ID defining the relative volume change
(change in volume relative to the initial volume) as a function of
the effective plastic strain.  This is only used when nonzero.  See
Remarks. 
Barlat89 parameter, p.  If PB > 0, parameters AB, CB, and HB are 
read instead of R00, R45, and R90.  See Remarks below. 
ID  of  a  load  curve  of  the  Forming  Limit  Diagram  (FLD)  under
linear  strain  paths.    In  the  load  curve,  abscissas  represent  minor 
strains while ordinates represent major strains.  Define only when
option NLP is used.  See Remarks. 
Load  curve/Table  ID  for  postforming  parameter  A  in  heat
treatment 
Load  curve/Table  ID  for  postforming  parameter  B  in  heat 
treatment 
XP, YP, ZP 
Coordinates of point 𝐩 for AOPT = 1. 
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2. 
HTC 
HTD 
Load  curve/Table  ID  for  postforming  parameter  C  in  heat
treatment 
Load  curve/Table  ID  for  postforming  parameter  D  in  heat 
treatment 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3. 
D1, D2, D3 
Components of vector 𝐝 for AOPT = 2.
VARIABLE   
BETA 
DESCRIPTION
Material angle in degrees for AOPT = 0 and 3, may be overridden 
on the element card, see *ELEMENT_SHELL_BETA. 
HTFLAG 
Heat treatment flag : 
HTFLAG.EQ.0:  Preforming stage 
HTFLAG.EQ.1:  Heat treatment stage 
HTFLAG.EQ.2:  Postforming stage 
USRFAIL 
User defined failure flag  
USRFAIL.EQ.0:  no user subroutine is called 
USRFAIL.EQ.1:  user subroutine matusr_24 in dyn21.f is called 
HR.EQ.7: Load  curve  defining  biaxial  stress  vs.    biaxial  strain
for hardening rule, see discussion in the formulation
section below for a definition. 
HR.NE.7:  Ignored. 
HR.EQ.7: Load curve defining shear stress vs.  shear strain for
hardening,  see  discussion  in  the  formulation  section
below for a definition. 
HR.NE.7:  Ignored. 
LCBI 
LCSH 
Formulation: 
The effective plastic strain used in this model is defined to be plastic work equivalent.  
A  consequence  of  this  is  that  for  parameters  defined  as  functions  of  effective  plastic 
strain, the rolling (00) direction should be used as reference direction.  For instance, the 
hardening curve for HR = 3 is the stress as function of strain for uniaxial tension in the 
rolling  direction,  VLCID  curve  should  give  the  relative  volume  change  as  function  of 
strain  for  uniaxial  tension  in  the  rolling  direction  and  load  curve  given  by  -E  should 
give  the  Young’s  modulus  as  function  of  strain  for  uniaxial  tension  in  the  rolling 
direction.    Optionally,  the  curve  can  be  substituted  for  a  table  defining  hardening  as 
function of plastic strain rate (HR = 3) or temperature (HR = 8). 
Exceptions from the rule above are curves defined as functions of plastic strain in the 45 
and 90 directions, i.e., P1 and P2 for HR = 7 and negative R45 or R90, see Fleischer et.al.  
[2007].    The  hardening  curves  are  here  defined  as  measured  stress  as  function  of 
measured  plastic  strain  for  uniaxial  tension  in  the  direction  of  interest,  i.e.,  as 
determined from experimental testing using a standard procedure.  The optional biaxial
and  shear  hardening  curves  require  some  further  elaboration,  as  we  assume  that  a 
biaxial or shear test reveals that the true stress tensor in the material system expressed 
as 
is a function of the (plastic) strain tensor 
𝝈 = (
0 ±𝜎
) ,
𝜎 ≥ 0, 
𝜺 = (
𝜀1
0 ±𝜀2
) ,
𝜀1 ≥ 0,
𝜀2 ≥ 0, 
The input hardening curves are 𝜎 as function of 𝜀1+𝜀2.  The ± sign above distinguishes 
between  the  biaxial  (+)  and  the  shear  (−)  cases.    Moreover,  the  curves  defining  the  R 
values are as function of the measured plastic strain for uniaxial tension in the direction 
of interest.  These curves are transformed internally to be used with the effective stress 
and strain properties in the actual model.  The effective plastic strain does not coincide 
with the plastic strain components in other directions than the rolling direction and may 
be  somewhat  confusing  to  the  user.    Therefore  the  von  Mises  work  equivalent  plastic 
strain  is  output  as  history  variable  #2  if  HR = 7  or  if  any  of  the  R-values  is  defined  as 
function of the plastic strain. 
The  R-values  in  curves  are  defined  as  the  ratio  of  instantaneous  width  change  to 
instantaneous thickness change.  That is, assume that the width W and thickness T are 
measured as function of strain.  Then the corresponding R-value is given by: 
𝑅 =
𝑑𝑊
𝑑𝜀
𝑑𝑇
𝑑𝜀
/𝑊
/𝑇
The anisotropic yield criterion Φ for plane stress is defined as: 
𝑚 
Φ = 𝑎|𝐾1 + 𝐾2|𝑚 + 𝑎|𝐾1 − 𝐾2|𝑚 + 𝑐|2𝐾2|𝑚 = 2𝜎𝑌
where 𝜎𝑌 is the yield stress and Ki = 1,2 are given by: 
𝐾1 =
𝜎𝑥 + ℎ𝜎𝑦
√
√√
⎷
𝐾2 =
(
𝜎𝑥 − ℎ𝜎𝑦
)
2  
+ 𝑝2𝜏𝑥𝑦
If PB = 0, the anisotropic material constants a, c, h, and p are obtained through R00, R45, 
and R90: 
𝑎 = 2 − 2√(
𝑅00
1 + 𝑅00
) (
𝑅90
1 + 𝑅90
) 
𝑐 = 2 − 𝑎
ℎ = √(
𝑅00
1 + 𝑅00
) (
1 + 𝑅90
𝑅90
) 
The anisotropy parameter p is calculated implicitly.  According to Barlat and Lian the R 
value, width to thickness strain ratio, for any angle 𝜙 can be calculated from: 
𝑅𝜙 =
2𝑚𝜎𝑌
+ ∂Φ
∂𝜎𝑦
(∂Φ
∂𝜎𝑥
) 𝜎𝜙
− 1 
where  𝜎𝜙  is  the  uniaxial  tension  in  the  𝜙  direction.    This  expression  can  be  used  to 
iteratively calculate the value of p.  Let 𝜙 = 45 and define a function 𝑔 as: 
𝑔(𝑝) =
2𝑚𝜎𝑌
+ ∂Φ
∂𝜎𝑦
(∂Φ
∂𝜎𝑥
) 𝜎𝜙
− 1 − 𝑅45 
An iterative search is used to find the value of p.  If PB > 0, material parameters a (AB), 
c (CB), h (HB), and p (PB) are used directly. 
For  face  centered  cubic  (FCC)  materials  m = 8  is  recommended  and  for  body  centered 
cubic  (BCC)  materials  m = 6  may  be  used.    The  yield  strength  of  the  material  can  be 
expressed in terms of k and n: 
𝜎𝑦 = 𝑘𝜀𝑛 = 𝑘(𝜀𝑦𝑝 + 𝜀̅𝑝)
where 𝜀𝑦𝑝 is the elastic strain to yield and 𝜀̅𝑝is the effective plastic strain (logarithmic).  
If  SIGY  is  set  to  zero, the  strain  to yield  if  found  by  solving  for the  intersection  of  the 
linearly elastic loading equation with the strain hardening equation: 
𝜎 = 𝐸𝜀 
𝜎 = 𝑘𝜀𝑛 
which gives the elastic strain at yield as: 
If SIGY yield is nonzero and greater than 0.02 then: 
𝜀𝑦𝑝 = (
𝑛−1
)
𝜀𝑦𝑝 = (
𝜎𝑦
)
The other available hardening models include the Voce equation given by: 
the Gosh equation given by: 
𝜎Y(𝜀𝑝) = 𝑎 − 𝑏𝑒−𝑐𝜀𝑝, 
𝜎Y(𝜀𝑝) = 𝑘(𝜀0 + 𝜀𝑝)𝑛 − 𝑝, 
and finally the Hocket-Sherby equation given by:
𝜎Y(𝜀𝑝) = 𝑎 − 𝑏𝑒−𝑐𝜀𝑝
. 
For the Gosh hardening law, the interpretation of the variable SPI is the same, i.e., if set 
to  zero  the  strain  at  yield  is  determined  implicitly  from  the  intersection  of  the  strain 
hardening equation with the linear elastic equation. 
To  include  strain  rate  effects  in  the  model  we  multiply  the  yield  stress  by  a  factor 
depending  on  the  effective  plastic  strain  rate.    We  use  the  Cowper-Symonds’  model, 
hence the yield stress can be written as: 
1/𝑝
𝜀̇𝑝
1 + (
𝑠 (𝜀𝑝)
𝜎Y(𝜀𝑝, 𝜀̇𝑝) = 𝜎Y
{⎧
⎩{⎨
𝑠   denotes  the  static  yield  stress,  𝐶  and  𝑝  are  material  parameters,  𝜀̇𝑝   is  the 
where  𝜎Y
effective plastic strain rate.  It is also possible to use a table with HR.EQ.3 for defining 
the strain rate effects, for which each load curve in the table defines the yield stress as 
function of plastic strain for a given strain rate.  In contrast to material 24, whenever the 
strain rate is higher than that of any curve in the table, the table is extrapolated in the 
strain rate direction to find the appropriate yield stress.  
}⎫
⎭}⎬
)
A  kinematic  hardening  model  is  implemented  following  the  works  of  Chaboche  and 
Roussilier.  A back stress α is introduced such that the effective stress is computed as: 
𝜎eff = 𝜎eff(𝜎11 − 2𝛼11 − 𝛼22, 𝜎22 − 2𝛼22 − 𝛼11, 𝜎12 − 𝛼12) 
The back stress is the sum of up to four terms according to: 
𝛼𝑖𝑗 = ∑ 𝛼𝑖𝑗
𝑘=1
and the evolution of each back stress component is as follows: 
𝛿𝛼𝑖𝑗
𝑘 = 𝐶𝑘 (𝑎𝑘
𝑠𝑖𝑗
𝜎eff
− 𝛼𝑖𝑗
𝑘 ) 𝛿𝜀𝑝 
where  𝐶𝑘  and  𝑎𝑘  are  material  parameters,𝑠𝑖𝑗  is  the  deviatoric  stress  tensor,  𝜎eff  is  the 
effective stress and 𝜀𝑝 is the effective plastic strain.  The yield condition is for this case 
modified according to 
𝑓 (σ,α, 𝜀𝑝) = 𝜎eff(𝜎11 − 2𝛼11 − 𝛼22, 𝜎22 − 2𝛼22 − 𝛼11, 𝜎12 − 𝛼12)
− {𝜎𝑌
𝑡 (𝜀𝑝, 𝜀̇𝑝, 0) − ∑ 𝑎𝑘[1 − exp(−𝐶𝑘𝜀𝑝 ]
} ≤ 0 
in order to get the expected stress strain response for uniaxial stress. 
The calculated effective stress is stored in history variable #7. 
𝑘=1
A Failure Criterion For Nonlinear Strain Paths (NLP) in sheet metal forming: 
When the option NLP is used, a necking failure criterion is activated to account for the 
non-linear strain path effect in sheet metal forming.  Based on the traditional Forming 
Limit Diagram (FLD) for the linear strain path, the Formability Index (F.I.) is calculated 
for every element in the model throughout the simulation duration.  The entire F.I.  time 
history for every element is stored in history variable #1 in d3plot files, accessible from 
Post/History  menu  in  LS-PrePost  v4.0.    In  addition  to  the  F.I.    output,  other  useful 
information stored in other history variables can be found as follows, 
1.  Formability Index: #1 
2.  Strain ratio (in-plane minor strain/major strain): #2 
3.  Effective strain from the planar isotropic assumption: #3 
To enable the output of these history variables to the d3plot files, NEIPS on the *DATA-
BASE_EXTENT_BINARY card must be set to at least 3.  The history variables can also 
be  plotted  on  the  formed  sheet  blank  as  a  color  contour  map,  accessible  from 
Post/FriComp/Misc  menu.    The  index  value  starts  from  0.0,  with  the  onset  of  necking 
failure when it reaches 1.0.  The F.I.  is calculated based on critical effect strain method, 
as illustrated in a figure in Remarks section in *MAT_037.  The theoretical background 
can be found in two papers also referenced in Remarks section in *MAT_037. 
When d3plot files are used to plot the history variable #1 (the F.I.) in color contour, the 
value in the “Max” pull-down menu in Post/FriComp needs to be set to “Min”, meaning 
that  the  necking  failure  occurs  only  when  all  integration  points  through  the  thickness 
have reached the critical value of 1.0 (refer to Tharrett and Stoughton’s paper in 2003 SAE 
2003-01-1157).  It is also suggested to set the variable “MAXINT” in *DATABASE_EX-
TENT_BINARY  to  the  same  value  as  the  variable  “NIP”  in  *SECTION_SHELL.    In 
addition,  the  value  in  the  “Avg”  pull-down  menu  in  Post/FriRang  needs  to  be  set  to 
“None”.  The strain path history (major vs.  minor strain) of each element can be plotted 
with the radial dial button Strain Path in Post/FLD. 
An example of a partial input for the material is provided below, where the FLD for the 
linear  strain  path  is  defined  by  the  variable  NLP  with  load  curve  ID  211,  where 
abscissas represent minor strains and ordinates represent major strains. 
*MAT_3-PARAMETER_BARLAT_NLP 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
$      MID        RO         E        PR        HR        P1        P2      ITER 
         1 2.890E-09  6.900E04     0.330     3.000                     
$        M       R00       R45       R90      LCID        E0       SPI        P3 
     8.000     0.800     0.600     0.550        99 
$     AOPT         C         P     VLCID                           NLP 
     2.000                                                         211 
$                                     A1        A2        A3 
                                   0.000     1.000     0.000 
$       V1        V2        V3        D1        D2        D3      BETA
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
$ Hardening Curve 
*DEFINE_CURVE 
        99 
               0.000             130.000 
               0.002             134.400 
               0.006             143.000 
               0.010             151.300 
               0.014             159.300 
                 ⋮                   ⋮ 
               0.900             365.000 
               1.000             365.000 
$ FLD Definition 
*DEFINE_CURVE 
211 
                -0.2               0.325 
             -0.1054              0.2955 
             -0.0513              0.2585 
              0.0000              0.2054 
              0.0488              0.2240 
              0.0953              0.2396 
              0.1398              0.2523 
              0.1823              0.2622 
                 ⋮                    ⋮ 
Shown in Figures M36-1, M36-2 and M36-3, predictions and validations of forming limit 
curves (FLC) of various nonlinear strain paths on a single shell element was done using 
this  new  option,  for  an  Aluminum  alloy  with  r00 = 0.8,  r45 = 0.6,  r90 = 0.55,  and  yield  at 
130.0 MPa.  In each case, the element is further strained in three different paths (uniaxial 
stress – U.A., plane strain – P.S., and equi-biaxial strain – E.B.)  separately, following a 
pre-straining  in  uniaxial,  plane  strain  and  equi-biaxial  strain  state,  respectively.    The 
forming limits are determined at the end of the secondary straining for each path, when 
the F.I.  has reached the value of 1.0.  It is seen that the predicted FLCs (dashed curves) 
in case of the nonlinear strain paths are totally different from the FLCs under the linear 
strain paths.  It is noted that the current predicted FLCs under nonlinear strain path are 
obtained  by  connecting  the  ends  of  the  three  distinctive  strain  paths.    More  detailed 
FLCs can  be obtained  by straining the elements in more paths  between U.A.  and P.S.  
and between P.S.  and E.B.  In Figure M36-4, time-history plots of F.I., strain ratio and 
effective strain are shown for uniaxial pre-strain followed by equi-biaxial strain path on 
the same single element. 
Typically, to assess sheet formability, F.I.  contour of the entire part should be plotted.  
Based  on  the  contour  plot,  non-linear  strain  path  and  the  F.I.    time  history  of  a  few 
elements in the area of concern can be plotted for further study.  These plots are similar 
to those shown in manual pages of *MAT_037. 
Heat treatment with variable HTFLAG: 
Heat  treatment  for  increasing  the  formability  of  prestrained  aluminum  sheets  can  be 
simulated  through  the  use  of  HTFLAG,  where  the  intention  is  to  run  a  forming 
simulation in steps involving preforming, springback, heat treatment and postforming.
In  each  step  the  history  is  transferred  to  the  next  via  the  use  of  dynain  .  The first two steps are performed with HTFLAG = 0 according 
0corresponding  to  the 
to  standard  procedures,  resulting  in  a  plastic  strain  field  𝜀𝑝
prestrain.    The  heat  treatment  step  is  performed  using  HTFLAG = 1  in  a  coupled 
thermomechanical  simulation,  where  the  blank  is  heated.    The  coupling  between 
thermal and mechanical is only that the maximum temperature 𝑇0 is stored as a history 
variable  in  the  material  model,  this  corresponding  to  the  heat  treatment  temperature.  
Here it is important to export all history variables to the dynein file for the postforming 
step.  In the final postforming step, HTFLAG = 2, the yield stress is then augmented by 
the Hocket-Sherby like term: 
0)
Δ𝜎 = 𝑏 − (𝑏 − 𝑎)exp[−𝑐(𝜀𝑝 − 𝜀𝑝
] 
where a, b, c and d are given as tables as functions of the heat treatment temperature 𝑇0 
0. That is, in the table definitions each load curve corresponds to a given 
and prestrain 𝜀𝑝
prestrain and the load curve value is with respect to the heat treatment temperature, 
𝑎 = 𝑎(𝑇0, 𝜀𝑝
0)    𝑏 = 𝑏(𝑇0, 𝜀𝑝
0)    𝑐 = 𝑐(𝑇0, 𝜀𝑝
0)    𝑑 = 𝑑(𝑇0, 𝜀𝑝
0)     
The  effect  of  heat  treatment  is  that  the  material  strength  decreases  but  hardening 
increases, thus typically: 
𝑎 ≤ 0    𝑏 ≥ 𝑎    𝑐 > 0    𝑑 > 0     
Revision information: 
The option NLP is available in explicit dynamic analysis and in SMP and MPP, starting 
in Revision 95576.
Fx 0=
n i- a
x i a l str e s s
Fx 0=
uy
P la n e str ai n
uy
Fx 0=
n i- a
x i a l str e s s
Fx 0=
uy
u i- b ia x ial
uy
ux
uy=
n str a i n
e ll
 s h
FLC- nonlinear strain path
FLC- linear strain path
0.35
0.30
0.25
0.20
0.15
0.10
0.05
U.A.
P.S.
E.B.
U.A.
-0.2
-0.1
0.1
Minor true strain
0.2
Figure M36-1.  Nonlinear FLD prediction with uniaxial pre-straining.
Fx 0=
n i- a
x i a l str e s s
Fx 0=
uy
P la n e str ai n
uy
P la n e str ai n
uy
u i- b ia x ial
uy
ux
uy=
n str a i n
e ll
 s h
FLC- nonlinear strain path
FLC- linear strain path
0.35
0.30
0.25
0.20
0.15
0.10
0.05
U.A.
P.S.
E.B.
P.S.
-0.2
-0.1
0.1
Minor true strain
0.2
  Figure M36-2.  Nonlinear FLD prediction with plane strain pre-straining.
Fx 0=
n i- a
x i a l str e s s
Fx 0=
uy
P la n e str ai n
u i- b ia x ial
uy
ux
uy=
uy
u i- b ia x ial
uy
ux
uy=
n str a i n
e ll
 s h
FLC- nonlinear strain path
FLC- linear strain path
U.A.
E.B.
P.S.
E.B.
0.35
0.30
0.25
0.20
0.15
0.10
0.05
-0.2
-0.1
0.1
Minor true strain
0.2
  Figure M36-3.  Nonlinear FLD prediction with equi-biaxial pre-straining.
1.2
1.0
0.8
0.6
0.4
0.2
0.0
1.0
0.8
0.6
0.4
0.2
0.0
-0.2
-0.4
0.6
0.5
0.4
0.3
0.2
0.1
0.0
)
#
(
.
.
)
#
(
)
#
(
Uniaxial
Equi-biaxial
Time, seconds (E-03)
Uniaxial
Equi-biaxial
Time, seconds (E-03)
Uniaxial
Equi-biaxial
Time, seconds (E-03)
Figure M36-4.  Time-history plots of the three history variables.
*MAT_EXTENDED_3-PARAMETER_BARLAT 
This  is  Material  Type  36E.    This  model  is  an  extension  to  the  standard  3-parameter 
Barlat  model  and  allows  for  different  hardening  curves  and  R-values  in  different 
directions,  see  Fleischer  et.al.    [2007].    The  directions  in  this  context  are  the  three 
uniaxial directions (0, 45 and 90 degrees) and optionally biaxial and shear. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
E 
F 
3 
4 
PR 
F 
4 
5 
6 
7 
8 
5 
6 
7 
8 
Variable 
LCH00 
LCH45 
LCH90 
LCHBI 
LCHSH 
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
F 
4 
F 
5 
Variable 
LCR00 
LCR45 
LCR90 
LCRBI 
LCRSH 
F 
2 
F 
3 
Type 
F 
  Card 4 
1 
Variable 
AOPT 
Type 
F 
  Card 5 
1 
2 
3 
Variable 
Type 
2-270 (EOS) 
F 
4 
4 
A1 
F 
F 
5 
5 
A2 
F 
6 
M 
F 
6 
6 
A3 
F 
7 
8 
7 
8
Card 6 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
7 
8 
BETA 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
LCHXX 
LCHBI 
LCHSH 
LCRXX 
LCRBI 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus, 𝐸. 
Poisson’s ratio, ν. 
Load  curve  defining  uniaxial  stress  vs.    uniaxial  strain  in  the
given  direction  (XX  is  either  00, 45, 90).    The  exact  definition  is 
discussed  in  the  Remarks  below.    LCH00  must  be  defined,  the
other defaults to LCH00 if not defined. 
Load  curve  defining  biaxial  stress  vs. 
  biaxial  strain,  see 
discussion  in  the  Remarks  below  for  a  definition.    If  not  defined
this is determined from LCH00 and the initial R-values to yield a 
response close to the standard 3-parameter Barlat model. 
Load  curve  defining  shear  stress  vs.    shear  strain,  see  discussion
in  the  Remarks  below  for  a  definition.    If  not  defined  this  is
ignored  to  yield  a  response  close  to  the  standard  3-parameter 
Barlat model. 
Load  curve  defining  standard  R-value  vs.    uniaxial  strain  in  the 
given  direction  (XX  is  either  00,  45,  90).    The  exact  definition  is 
discussed in the Remarks below.  Default is a constant R-value of 
1.0, a negative input will result in a constant R-value of –LCRXX. 
Load  curve  defining  biaxial  R-value  vs.    biaxial  strain,  see 
discussion  in  the  Remarks  below  for  a  definition.    Default  is  a
constant R-value of 1.0, a negative input will result in a constant
R-value of –LCRBI.
LCRSH 
M 
AOPT 
*MAT_EXTENDED_3-PARAMETER_BARLAT 
DESCRIPTION
Load curve defining shear R-value vs.  shear strain, see discussion 
in  the  Remarks  below  for  a  definition.    Default  is  a  constant  R-
value of 1.0, a negative input will result in a constant R-value of –
LCRSH. 
Barlat flow exponent, 𝑚, must be an integer value. 
Material axes option : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES,  and  then  rotated  about  the  shell  ele-
ment normal by an angle BETA. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by 
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the
element normal. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).    Available  with  the  R3  release 
of Version 971 and later. 
XP, YP, ZP 
Coordinates of point 𝐩 for AOPT = 1. 
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3. 
D1, D2, D3 
Components of vector 𝐝 for AOPT = 2. 
BETA 
Material angle in degrees for AOPT = 0 and 3, may be overridden 
on the element card, see *ELEMENT_SHELL_BETA. 
Formulation: 
The hardening curves LCH00, LCH45 and LCH90 are here defined as measured stress 
as  function  of  measured  plastic  strain  for  uniaxial  tension  in  the  direction  of  interest,
i.e., as determined from experimental testing using a standard procedure.  The optional 
biaxial  and  shear  hardening  curves  LCHBI  and  LCHSH  require  some  further 
elaboration, as we assume that a biaxial or shear test reveals that the true stress tensor 
in the material system expressed as 
is a function of the (plastic) strain tensor 
𝝈 = (
0 ±𝜎
) ,
𝜎 ≥ 0, 
𝜺 = (
𝜀1
0 ±𝜀2
) ,
𝜀1 ≥ 0,
𝜀2 ≥ 0, 
The input hardening curves are 𝜎 as function of 𝜀1+𝜀2.  The ± sign above distinguishes 
between the biaxial (+) and the shear (−) cases. 
Moreover, the curves LCR00, LCR45 and LCR90 defining the R values are as function of 
the measured plastic strain for uniaxial tension in the direction of interest.  The R-values 
in  themselves  are  defined  as  the  ratio  of  instantaneous  width  change  to  instantaneous 
thickness  change.    That  is,  assume  that  the  width  W  and  thickness  T  are  measured  as 
function of strain.  Then the corresponding R-value is given by: 
𝑅𝜑 =
𝑑𝑊
𝑑𝜀
𝑑𝑇
𝑑𝜀
/𝑊
/𝑇
. 
These  curves  are  transformed  internally to  be  used  with  the  effective  stress  and  strain 
properties  in  the  actual  model.    The  effective  plastic  strain  does  not  coincide  with  the 
plastic  strain  components  in  other  directions  than  the  rolling  direction  and  may  be 
somewhat confusing to the user.  Therefore the von Mises work equivalent plastic strain 
is  output  as  history  variable  #2.    As  for  hardening,  the  optional  biaxial  and  shear  R-
value curves LCRBI and LCRSH are defined in a special way for which we return to the 
local plastic strain tensor 𝜺 as defined above.  The biaxial and shear R-values are defined 
as 
𝑅𝑏/𝑠 =
𝜀̇1
𝜀̇2
and again the curves are 𝑅𝑏/𝑠 as function of 𝜀1+𝜀2.  Note here that the suffix 𝑏 assumes 
loading  biaxially  and  𝑠  assumes  loading  in  shear,  so  the  R-values  to  be  defined  are 
always positive.
*MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLASTIC_{OPTION} 
This  is  Material  Type  37.    This  model  is  for  simulating  sheet  forming  processes  with 
anisotropic  material.    Only  transverse  anisotropy  can  be  considered.    Optionally  an 
arbitrary  dependency  of  stress  and  effective  plastic  strain  can  be  defined  via  a  load 
curve.  This plasticity model is fully iterative and is available only for shell elements.   
Available options include: 
<BLANK> 
ECHANGE 
NLP_FAILURE 
NLP2 
The ECHANGE option allows the change of Young’s Modulus during the simulation: 
The  NLP_FAILURE  option  estimates  failure  using  the  Formability  Index  (F.I.)  which 
accounts  for  the  non-linear  strain  paths  common  in  metal  forming  application  .  The option NLP is also available in *MAT_036, *MAT_125 and *MAT_226. 
The  NLP_FAULURE  option  uses  effective  plastic  strain  to  calculate  the  onset  of 
necking,  which  assumes  the  necking  happens  in  an  instant.    Some researchers  think  it 
may happen in a longer duration, which can be addressed by the option NLP2, which 
calculates  the  damage  during  forming  and  accumulates  it  to  predict  the  sheet  metal 
failure.  Compared with NLP_FAILURE, there is no input change required. 
  Card 1 
1 
Variable 
MID 
Type 
A 
2 
RO 
F 
3 
E 
F 
4 
PR 
F 
5 
6 
SIGY 
ETAN 
F 
F 
7 
R 
F 
8 
HLCID 
F 
Additional card for ECHANGE and/or NLP_FAILURE keyword options. 
  Card 2. 
1 
Variable 
IDSCALE 
Type 
I 
2 
EA 
F 
3 
4 
5 
6 
7 
8 
COE 
ICFLD 
STRAINLT 
F 
F
VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
SIGY 
ETAN 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
Yield stress. 
Plastic  hardening  modulus.    When  this  value  is  negative,  normal
stresses  (either  from  contact  or  applied  pressure)  are  considered
and  *LOAD_SURFACE_STRESS  must  be  used  to  capture  the 
stresses. 
The negative local 𝑧-stresses caused by the contact pressure can be 
viewed  from  d3plot  files  after  Revision  97158.    This  data  can  be 
viewed in LS-PrePost by selecting 𝑧-stress under FCOMP → Stress
and  select  local  under  FCOMP  in  LS-PrePost).    Prior  to  Revision 
97158, the negative local 𝑧-stresses are stored in history variable #5, 
and can be viewed with menu options FCOMP → Misc → history 
var  #5  in  LS-PrePost.    This  feature  is  applicable  to  both  shell 
element  types  2  and  16.    It  is  found  in  some  cases  this  inclusion
can improve forming simulation accuracy. 
R 
Anisotropic parameter, also commonly call r-bar, 𝑟 ̅, in sheet metal 
forming literature.  Its interpretation is given here. 
GT.0: Standard formulation. 
LT.0:  The anisotropic parameter is set to |R|.  When R is set to
a negative value the algorithm is modified for better sta-
bility in sheet thickness or thinning for sheet metal form-
ing  involving  high  strength  steels  or  in  cases  when  the
simulation  time  is  long.    This  feature  is  available  to  both
element  formulations  2  and  16.    An  example  using  this 
feature  is  provided  in  Remarks,  and  shown  in  Figure 
M37-4. 
HLCID 
Load  curve  ID  expressing  effective  yield  stress  as  a  function  of
effective plastic strain in uniaxial tension.
IDSCALE 
EA, COE 
ICFLD 
*MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLASTIC 
DESCRIPTION
Load curve ID expressing the scale factor for the Young’s modulus
as  a  function  of  effective  strain.    If  the  EA  and  COE  fields  are
specified,  this  curve  is  unnecessary.    This  field  is  only  used  and
should only be specified when the option ECHANGE is active. 
Coefficients  defining  the  Young’s  modulus  with  respect  to  the
effective  strain,  EA  is  𝐸𝐴  and  COE  is 𝜁 .    If  IDSCALE  is  defined, 
these  two  parameters  are  not  necessary.    Input  only  when  the
option ECHANGE is used.  Also see *MAT_125 for an example to
obtain these two coefficients from a test curve. 
ID  of  a  load  curve  of  the  Forming  Limit  Diagram  (FLD)  under
linear  strain  paths  .    In  the  load  curve,  abscissas 
represent  minor  strains  while  ordinates  represent  major  strains.
Define only when the option NLP_FAILURE is active. 
STRAINLT 
Critical strain value at which strain averaging is activated.  Input 
only when the option NLP_FAILURE is active.  See Remarks. 
Formulation: 
Consider  Cartesian  reference  axes  which  are  parallel  to  the  three  symmetry  planes  of 
anisotropic behavior.  Then, the yield function suggested by Hill [1948] can be written 
as: 
𝐹(𝜎22 − 𝜎33)2 + 𝐺(𝜎33 − 𝜎11)2 + 𝐻(𝜎11 − 𝜎22)2 + 2𝐿𝜎23
2 + 2𝑀𝜎31
2 + 2𝑁𝜎12
2 − 1 = 0 
where  𝜎𝑦1,  𝜎𝑦2,  and  𝜎𝑦3,  are  the  tensile  yield  stresses  and  𝜎𝑦12,  𝜎𝑦23,  and  𝜎𝑦31  are  the 
shear yield stresses.  The constants F, G H, L, M, and N are related to the yield stress by: 
2𝐿 =
2𝑀 =
2𝑁 =
2  
𝜎𝑦23
2  
𝜎𝑦31
2  
𝜎𝑦12
2𝐹 =
 2 +
𝜎𝑦2
 2 −
𝜎𝑦3
 2  
𝜎𝑦1
2𝐺 =
 2 +
𝜎𝑦3
 2 −
𝜎𝑦1
 2  
𝜎𝑦2
2𝐻 =
 2 +
𝜎𝑦1
 2 −
𝜎𝑦2
 2   . 
𝜎𝑦3
The isotropic case of von Mises plasticity can be recovered by setting: 
and  
𝐹 = 𝐺 = 𝐻 =
𝐿 = 𝑀 = 𝑁 =
2 
2𝜎𝑦
2 
2𝜎𝑦
For the particular case of transverse anisotropy, where properties do not vary in the x1-
x2 plane, the following relations hold: 
2𝐹 = 2𝐺 =
2  
𝜎𝑦3
2𝐻 =
2 −
𝜎𝑦
2  
𝜎𝑦3
𝑁 =
2 −
𝜎𝑦
2  
𝜎𝑦3
where it has been assumed that 𝜎𝑦1 = 𝜎𝑦2 = 𝜎𝑦. 
Letting 𝐾 =
𝜎𝑦
𝜎𝑦3
, the yield criteria can be written as: 
𝐹(𝜎) = 𝜎𝑒 = 𝜎𝑦, 
where, 
𝐹(𝜎) ≡ [𝜎11
2 + 𝜎22
2 + 𝐾2𝜎33
2 − 𝐾2𝜎33(𝜎11 + 𝜎22) − (2 − 𝐾2)𝜎11𝜎22 + 2𝐿𝜎𝑦
2(𝜎23
2 )
2 + 𝜎31
+ 2 (2 −
2 ]
𝐾2) 𝜎12
2⁄
. 
The  rate  of  plastic  strain  is  assumed  to  be  normal  to  the  yield  surface  so  𝜀̇𝑖𝑗
from: 
𝑝  is  found 
𝑝 = 𝜆
𝜀̇𝑖𝑗
∂𝐹
∂𝜎𝑖𝑗
. 
Now consider the case of plane stress, where σ33 = 0.  Also, define the anisotropy input 
parameter,  R,  as  the  ratio  of  the  in-plane  plastic  strain  rate  to  the  out-of-plane  plastic 
strain rate, 
𝑅 =
𝜀̇22
𝑝 . 
𝜀̇33
It then follows that
𝑅 =
𝐾2 − 1. 
Using the plane stress assumption and the definition of R, the yield function may now 
be written as: 
𝐹(𝜎) = [𝜎11
2 + 𝜎22
2 −
2𝑅
𝑅 + 1
𝜎11𝜎22 + 2
2𝑅 + 1
𝑅 + 1
2⁄
. 
2 ]
𝜎12
Discussion and ECHANGE: 
It  is  noted  that  there  are  several  differences  between  this  model  and  other  plasticity 
models  for  shell  elements  such  as  the  model,  MAT_PIECEWISE_LINEAR_PLASTICI-
TY.  First, the yield function for plane stress does not include the transverse shear stress 
components  which  are  updated  elastically,  and,  secondly,  this  model  is  always  fully 
iterative.  Consequently, in comparing results for the isotropic case where R = 1.0 with 
other  isotropic  model,  differences  in  the  results  are  expected,  even  though  they  are 
usually insignificant. 
The  Young’s  modulus  has  been  assumed  to  be  constant.    Recently,  some  researchers 
have  found  that  Young’s  modulus  decreases  with  respect  to  the  increase  of  effective 
strain.    To  accommodate  this  new  observation,  a  new  option  of  ECHANGE  is  added.  
There are two methods defining the change of Young’s modulus change: 
The first method is to use a curve to define the scale factor with respect to the effective 
strain.    The  value  of  this  scale  factor  should  decrease  from  1  to  0  with  the  increase  of 
effective strain. 
The second method is to use a function as proposed by Yoshida [2003]: 
𝐸 = 𝐸0 − (𝐸0 − 𝐸𝐴)[1 − exp(−𝜁 𝜀)]. 
An example of the option ECHANGE is provided in the Remarks section of the *MAT_-
125 manual pages. 
A Failure Criterion for Nonlinear Strain Paths (NLP): 
Background and Definition. 
When  the  option  NLP_FAILURE  is  used,  a  necking  failure  criterion  independent  of 
strain path changes is activated.  In sheet metal forming, as strain path history (plotted 
on  in-plane  major  and  minor  strain  space)  of  an  element  becomes  non-linear,  the 
position and shape of a traditional strain-based Forming Limit Diagram (FLD) changes.
This  option  provides  a  simple  formability  index  (F.I.)  which  remains  invariant 
regardless of the presence of the non-linear strain paths in the model, and can be used 
to identify if the element has reached its necking limit. 
0.4
0.3
0.2
0.1
-0.5
F.I. = Y / YL
YL
0.1
1.0
β = dε2 / dε1
  Figure M37-1.  Calculation of F.I.  based on critical effective strain method. 
Formability index (F.I) is calculated, as illustrated in Figure M37-1, for every element in 
the sheet blank throughout the simulation duration.  The value of F.I.  is 0.0 for virgin 
material  and  reaches  maximum  of  1.0  when  the  material  fails.    The  theoretical 
background  can  be  found  in  two  papers:  1)  T.B.    Stoughton,  X.    Zhu,  “Review  of 
Theoretical  Models  of  the  Strain-Based  FLD  and  their  Relevance  to  the  Stress-Based  FLD, 
International  Journal  of  Plasticity”,  V.    20,  Issues  8-9,  P.    1463-1486,  2003;  and  2)  Danielle 
Zeng,  Xinhai  Zhu,  Laurent  B.    Chappuis,  Z.    Cedric  Xia,    “A  Path  Independent  Forming 
Limited  Criterion  for  Sheet  Metal  Forming  Simulations”,  2008  SAE  Proceedings,  Detroit  MI, 
April, 2008.  
Required inputs. 
The  load  curve  input  for  ICFLD  follows  keyword  format  in  *DEFINE_CURVE,  with 
abscissas as minor strains and ordinates as major strains. 
ICFLD can also be specified using the *DEFINE_CURVE_FLC keyword where the sheet 
metal thickness and strain hardening value are used.  Detailed usage information can be 
found in the manual entry for *DEFINE_CURVE_FLC. 
The formability index is output as a history variable #1 in d3plot files.  In addition to the 
F.I.  values, starting in Revision 95599, the strain ratio 𝛽 and effective plastic strain 𝜀̅ are 
written  to  the  d3plot  database  as  history  variables  #2  and  #3,  respectively  provided 
NEIPS on the second field of the first card of *DATABASE_EXTENT_BINARY is set to
at least 3.  The contour map of history variables can be plotted in LS-PrePost, accessible 
in Post/FriComp, under Misc, and by Element, under Post/History. 
Post-processing information. 
When  plotting  the  formability  index  contour  map,  first  select  the  history  var  #1  from 
Misc in the FriComp menu.  The  pull-down  menu under FriComp can be  used to select 
the minimum value “Min” for necking failure detection (refer to Tharrett and Stoughton’s 
paper  in  2003  SAE  2003-01-1157).    In  the  FriRang  dialog,  select  None  on  the  pull-down 
menu next to “Avg”.  Lastly, set the simulation result to the last state on the animation 
tool bar.  The index value ranges from 0.0 to 1.5.  The non-linear forming limit is reached 
at 1.0. 
In addition, the evolution of the index throughout the simulation can be plotted in LS-
PrePost4.0 under Post/History by Element.  Select the last entry, which is history var#1 it 
may  be  hidden  by  a  scroll  bar.    Furthermore,  the  strain  path  of  an  element  can  be 
plotted in Post/FLD, using the Tracer option, by selecting the corresponding integration 
point representing the “Min” index value in the Position pull-down menu. 
Similarly  contour  maps  and  the  evolution  of  the  strain  ratio  and  the  effective  plastic 
strain can be plotted in the same way using variables 2 and 3. 
By  setting  the  STRAINLT  field  strains  (and  strain  ratios)  can  be  averaged  to  reduce 
noise,  which,  in  turn,  affect  the  calculation  of  the  formability  index.    The  strain 
STRAINLT  causes  the  formability  index  calculation  to  use  only  time  averaged  strains.  
Reasonable STRAINLT values range from 5 × 10−3 to 10−2. 
It  is  suggested  that  variable  “MAXINT”  in  *DATABASE_EXTENT_BINARY  be  set  to 
the same value of as the “NIP” field for the *SECTION_SHELL keyword. 
Input example. 
An example of a partial keyword input using this non-linear strain path failure criterion 
is provided below: 
*KEYWORD 
... 
*DATABASE_EXTENT_BINARY 
$    NEIPH     NEIPS    MAXINT    STRFLG    SIGFLG    EPSFLG    RLTFLG    ENGFLG 
                   3      &nip         1 
$   CMPFLG    IEVERP    BEAMIP     DCOMP      SHGE     STSSZ 
                   1                   2
... 
*MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLASTIC_NLP_FAILURE 
$      MID        RO         E        PR      SIGY      ETAN         R  HLCID 
         1 7.830E-09 2.070E+05      0.28       0.0       0.0     0.864    200 
$      IDY        EA       COE     ICFLD            STRAINLT 
                                     891             1.0E-02 
*DEFINE_CURVE 
891 
$ minor, major strains for FLD definition 
       -3.375000e-01        4.965000e-01 
       -2.750000e-01        4.340000e-01 
       -2.250000e-01        3.840000e-01 
       -1.840909e-01        3.430909e-01 
       -1.500000e-01        3.090000e-01 
       -1.211539e-01        2.801539e-01 
       -9.642858e-02        2.554286e-01 
       -7.500000e-02        2.340000e-01 
       -5.625001e-02        2.152500e-01 
       -3.970589e-02        1.987059e-01 
       -2.500000e-02        1.840000e-01 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ load curve  200: Mat_037 property, DP600 NUMISHEET'05 Xmbr, Power law fit 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
*DEFINE_CURVE 
200 
0.000,395.000 
0.001,425.200  
0.003,440.300  
0.004,452.000  
0.005,462.400  
0.006,472.100 
As  shown  in  Figure  M37-2,  F.I  contours  can  be  plotted  using  FriComp/Misc,  in  LS-
PrePost4.0.    Strain  paths  of  individual  elements,  or  elements  in  an  area  can  be  plotted 
(Figure  M37-3  left)  using  the  “Tracer”  feature  in  the  FLD  menu.    Finally,  time  history 
plot  of  the  formability  index  for  elements  selected  can  be  plotted  in  History  menu, 
Figure M37-3 right. 
Thickness/Thinning Stabilization for Shell Types 2 and 16: 
When the 𝑅 value is set to a negative value, it stabilizes the sheet thickness or thinning 
in  sheet  metal  forming  for  some  high  strength  types  of  steel  or  in  cases  where  the 
simulation time is long.  In Figure M37-4, a comparison of thinning contours is shown 
on  a  U-channel  forming  (one-half  model)  using  negative  and  positive  R  values.  
Maximum thinning on the draw wall is slight higher in the negative R case than that in 
the positive R case. 
Revision information: 
1)The  NLP_FAILURE  option  is  implemented  in  explicit  dynamic  and  is  available 
starting in Revision 60925. 
2)The maximum F.I.  value is change from 1.0 to 1.5 starting in Revision 72219.
3)The NLP_FAILURE option is also available starting in Revision 73241 for implicit 
static calculation. 
4)History variables #2 and #3 output is available starting in Revision 95599. 
in  d3plot 
5)Local 
*LOAD_SURFACE_STRESS) is available starting in Revision 97158. 
stress  output 
(when  used 
files 
𝑧 
together  with 
6)Negative 𝐸 option (contact pressure/normal stress) activated in formability index 
starts in Revision 97296. 
7)Numerical  material  model 
type  with 
the  NLP_FAILURE 
option 
(*MAT_037_NLP_FAULURE) is available starting in Revision 106898. 
8)Revision 111547: option NLP2.
Time = 0.1587, #nodes=476931
Contours of History Variable#1
min. ipt. value
min=0, at elem# 305
max=1, at elem# 8887
Formability
Index
1.0
0.9
0.8
0.7
0.6
0.5
0.4
0.3
0.2
0.1
Figure M37-2.  F.I.  contour plot (min IP value, non-averaged). 
0.60
0.50
0.40
0.30
0.20
0.10
-0.2
-0.1
0.1
Minor true strain
1.0
0.8
0.6
0.4
0.2
.
#
,
#
0.05
0.1
0.15
Time (sec.)
Nonlinear strain paths of a few elements in the box 
F.I. time history plots of the elements 
Figure  M37-3.    Strain  paths  and  F.I.    history  plot  for  elements  in  the  black
square box of the previous Figure.
Time=0.010271, #nodes=4594, #elem=4349
Contours of % Thickness Reduction based on current z-strain
min=0.0093799, at elem#42249
max=22.1816, at elem#39875
Time=0.010271, #nodes=4594, #elem=4349
Contours of % Thickness Reduction based on current z-strain
min=0.0597092, at elem#39814
max=21.2252, at elem#40457
Thinning %
20
18
16
14
12
10
With negative R-value
With positive R-value
Figure M37-4.  Thinning contour comparison.
*MAT_BLATZ-KO_FOAM 
*MAT_BLATZ-KO_FOAM 
*MAT_038 
This  is  Material  Type  38.    This  model  is  for  the  definition  of  rubber  like  foams  of 
polyurethane.  It is a simple one-parameter model with a fixed Poisson’s ratio of .25. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
G 
F 
4 
REF 
F 
5 
6 
7 
8 
  VARIABLE   
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Shear modulus. 
Use  reference  geometry  to  initialize  the  stress  tensor.    The
reference geometry is defined by the keyword:*INITIAL_FOAM_-
REFERENCE_GEOMETRY . 
EQ.0.0: off, 
EQ.1.0: on. 
MID 
RO 
G 
REF 
Remarks: 
The strain energy functional for the compressible foam model is given by  
𝑊 =
(
II
III
+ 2√III − 5) 
Blatz  and  Ko  [1962]  suggested  this  form  for  a  47  percent  volume  polyurethane  foam 
rubber with a Poisson’s ratio of 0.25.  In terms of the strain invariants, I, II, and III, the 
second Piola-Kirchhoff stresses are given as 
𝑆𝑖𝑗 = 𝐺 [(𝐼𝛿𝑖𝑗 − 𝐶𝑖𝑗)
III
+ (√III −
II
III
) 𝐶𝑖𝑗
−1] 
where Cij is the right Cauchy-Green strain tensor.  This stress measure is transformed to 
the Cauchy stress, σij, according to the relationship 
𝜎 𝑖𝑗 = III
−1
2⁄ 𝐹𝑖𝑘𝐹𝑗𝑙𝑆𝑙𝑘
where Fij is the deformation gradient tensor.
*MAT_FLD_TRANSVERSELY_ANISOTROPIC 
This  is  Material  Type  39.    This  model  is  for  simulating  sheet  forming  processes  with 
anisotropic  material.    Only  transverse  anisotropy  can  be  considered.    Optionally,  an 
arbitrary  dependency  of  stress  and  effective  plastic  strain  can  be  defined  via  a  load 
curve.    A  Forming  Limit  Diagram  (FLD)  can  be  defined  using  a  curve  and  is  used  to 
compute the maximum strain ratio which can be plotted in LS-PrePost.  This plasticity 
model  is  fully  iterative  and  is  available  only  for  shell  elements.    Also  see  the  notes 
below. 
2 
RO 
F 
2 
3 
E 
F 
3 
4 
PR 
F 
4 
5 
6 
SIGY 
ETAN 
F 
5 
F 
6 
7 
R 
F 
7 
8 
HLCID 
F 
8 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
Variable 
LCFLD 
Type 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
SIGY 
ETAN 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
Yield stress. 
Plastic hardening modulus, see notes for model 37. 
R 
Anisotropic hardening parameter, see notes for model 37. 
HLCID 
Load  curve  ID  defining  effective  stress  versus  effective  plastic
strain.  The yield stress and hardening modulus are ignored with
this option.
mjr = 0
mjr
Plane Strain
80
70
60
50
40
30
20
10
mnr
mjr
mnr
Draw
mjr
Stretch
%
-50
-40
-30
-20
-10
10
20
30
40
50
% Minor Strain
Figure M39-1.  Forming limit diagram. 
DESCRIPTION
Load  curve  ID  defining  the  Forming  Limit  Diagram.    Minor
strains in percent are defined as abscissa values and Major strains
in  percent  are  defined  as  ordinate  values.    The  forming  limit
diagram  is  shown  in  Figure  M39-1.    In  defining  the  curve  list 
pairs of minor and major strains starting with the left most point
and ending with the right most point, see *DEFINE_CURVE. 
  VARIABLE   
LCFLD 
Remarks: 
See  material  model  37  for  the  theoretical  basis.    The  first  history  variable  is  the 
maximum strain ratio: 
𝜀majorworkpiece
𝜀majorfld
. 
corresponding to 𝜀minorworkpiece.
*MAT_NONLINEAR_ORTHOTROPIC 
This is Material Type 40.  This model allows the definition of an orthotropic nonlinear 
elastic  material  based  on  a  finite  strain  formulation  with  the  initial  geometry  as  the 
reference.    Failure  is  optional  with  two  failure  criteria  available.    Optionally,  stiffness 
proportional  damping  can  be  defined.    In  the  stress  initialization  phase,  temperatures 
can be varied to impose the initial stresses.    This  model is only available for shell and 
solid elements. 
WARNING:  We do not recommend using this model at this 
time  since  it  can  be  unstable  especially  if  the 
stress-strain curves increase in stiffness with in-
creasing strain. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
EA 
F 
4 
EB 
F 
5 
EC 
F 
6 
7 
8 
PRBA 
PRCA 
PRCB 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
Variable 
GAB 
GBC 
GCA 
Type 
F 
F 
F 
Default 
none 
none 
none 
4 
DT 
F 
0 
5 
6 
7 
8 
TRAMP 
ALPHA 
F 
0 
F
Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCIDA 
LCIDB 
EFAIL 
DTFAIL 
CDAMP 
AOPT 
MACF 
Type 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 4 
Variable 
1 
XP 
Type 
F 
  Card 5 
Variable 
1 
V1 
Type 
F 
2 
YP 
F 
2 
V2 
F 
3 
ZP 
F 
3 
V3 
F 
4 
A1 
F 
4 
D1 
F 
5 
A2 
F 
5 
D2 
F 
6 
A3 
F 
6 
D3 
F 
I 
0 
7 
8 
7 
8 
BETA 
F 
Optional Card 6 (Applies to Solid elements only)  
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCIDC 
LCIDAB 
LCIDBC 
LCIDCA 
Type 
F 
F 
F 
F 
Default  optional  optional  optional optional
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density.
VARIABLE   
DESCRIPTION
EA 
EB 
EC 
PRBA 
PRCA 
PRCB 
GAB 
GBC 
GCA 
DT 
𝐸𝑎, Young’s modulus in 𝑎-direction. 
𝐸𝑏, Young’s modulus in 𝑏-direction. 
𝐸𝑐, Young’s modulus in 𝑐-direction. 
𝜈𝑏𝑎, Poisson’s ratio 𝑏𝑎. 
𝜈𝑏𝑎, Poisson’s ratio 𝑐𝑎. 
𝜈𝑐𝑏, Poisson’s ratio 𝑐𝑏. 
𝐺𝑎𝑏, shear modulus 𝑎𝑏. 
𝐺𝑏𝑐, shear modulus 𝑏𝑐. 
𝐺𝑐𝑎, shear modulus 𝑐𝑎. 
Temperature  increment  for  isotropic  stress  initialization.    This
option can be used during dynamic relaxation. 
TRAMP 
Time to ramp up to the final temperature. 
ALPHA 
Thermal expansion coefficient. 
LCIDA 
LCIDB 
Optional load curve ID defining the nominal  stress versus strain
along  𝑎-axis.    Strain  is  defined  as  𝜆𝑎 − 1  where  𝜆𝑎  is  the  stretch 
ratio along the 𝑎-axis. 
Optional load curve ID defining the nominal  stress versus strain
along  𝑏-axis.    Strain  is  defined  as  𝜆𝑏 − 1  where  𝜆𝑏  is  the  stretch 
ratio along the 𝑏-axis. 
EFAIL 
Failure strain, 𝜆 − 1. 
DTFAIL 
Time step for automatic element erosion 
CDAMP 
Damping coefficient. 
AOPT 
Material  axes  option  : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES, and then, for shells only, rotated about
the shell element normal by an angle BETA.
*MAT_NONLINEAR_ORTHOTROPIC 
DESCRIPTION
EQ.1.0: locally orthotropic with material axes determined by a 
point  in  space  and  the  global  location  of  the  element
center;  this  is  the  𝑎-direction.    This  option  is  for  solid 
elements only. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the 
element  normal.    The  plane  of  a  solid  element  is  the
midsurface between the inner surface and outer surface
defined by the first four nodes and the last four nodes
of the connectivity of the element, respectively. 
EQ.4.0: locally  orthotropic  in  cylindrical  coordinate  system 
with  the  material  axes  determined  by  a  vector  𝐯,  and 
an originating point, 𝐩, which define the centerline ax-
is.  This option is for solid elements only. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
MACF 
Material axes change flag: 
EQ.1: No change, default, 
EQ.2: switch material axes 𝑎 and 𝑏, 
EQ.3: switch material axes 𝑎 and 𝑐, 
EQ.4: switch material axes 𝑏 and 𝑐. 
XP, YP, ZP 
Define coordinates of point 𝐩 for AOPT = 1 and 4. 
A1, A2, A3 
(𝑎1, 𝑎2, 𝑎3) define components of vector 𝐚 for AOPT = 2. 
D1, D2, D3 
(𝑑1, 𝑑2, 𝑑3) define components of vector 𝐝 for AOPT = 2. 
V1, V2, V3 
(𝑣1, 𝑣2, 𝑣3) define components of vector 𝐯 for AOPT = 3 and 4.
VARIABLE   
BETA 
DESCRIPTION
Material  angle  in  degrees  for  AOPT = 0  (shells  only)  and 
AOPT = 3.      BETA  may  be  overridden  on  the  element  card,  see
*ELEMENT_SHELL_BETA and *ELEMENT_SOLID_ORTHO.. 
The following input is optional and applies to SOLID ELEMENTS only 
LCIDC 
LCIDAB 
LCIDBC 
LCIDCA 
Load  curve  ID  defining  the  nominal  stress  versus  strain  along  𝑐-
axis.  Strain is defined as 𝜆𝑐 − 1 where 𝜆𝑐 is the stretch ratio along 
the 𝑐-axis. 
Load  curve  ID  defining  the  nominal  ab  shear  stress  versus  𝑎𝑏-
strain in the 𝑎𝑏-plane.  Strain is defined as the sin(𝛾𝑎𝑏) where 𝛾𝑎𝑏
is the shear angle. 
Load  curve  ID  defining  the  nominal  ab  shear  stress  versus  𝑎𝑏-
strain in the 𝑏𝑐-plane.  Strain is defined as the sin(𝛾𝑏𝑐)where 𝛾𝑏𝑐 is 
the shear angle. 
Load  curve  ID  defining  the  nominal  ab  shear  stress  versus  𝑎𝑏-
strain in the 𝑐𝑎-plane.  Strain is defined as the sin(𝛾𝑐𝑎) where 𝛾𝑐𝑎 is 
the shear angle.
*MAT_USER_DEFINED_MATERIAL_MODELS 
These are Material Types 41 - 50.  The user must provide a material subroutine.  See also 
Appendix  A.    This  keyword  input  is  used  to  define  material  properties  for  the 
subroutine.    Isotopic,  anisotropic,  thermal,  and  hyperelastic  material  models  with 
failure can be handled. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
Variable 
MID 
RO 
MT 
LMC 
NHV 
IORTHO/ 
ISPOT 
IBULK 
Type 
A8 
  Card 2 
1 
F 
2 
I 
3 
I 
4 
I 
5 
I 
6 
Variable 
IVECT 
IFAIL 
ITHERM 
IHYPER 
IEOS 
LMCA 
Type 
I 
I 
I 
I 
I 
I 
Additional card for IORTHO = 1. 
  Card 3 
1 
2 
Variable 
AOPT 
MACF 
Type 
F 
I 
  Card 4 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
XP 
F 
3 
V3 
F 
4 
YP 
F 
4 
D1 
F 
5 
ZP 
F 
5 
D2 
F 
6 
A1 
F 
6 
D3 
F 
I 
7 
7 
A2 
F 
7 
8 
IG 
I 
8 
8 
A3 
F 
8 
BETA 
IEVTS 
F
Define LMC material parameters using 8 parameters per card.  
Card 
Variable 
1 
P1 
Type 
F 
2 
P2 
F 
3 
P3 
F 
4 
P4 
F 
5 
P5 
F 
6 
P6 
F 
Define LMCA material parameters using 8 parameters per card.  
Card 
Variable 
1 
P1 
Type 
F 
2 
P2 
F 
3 
P3 
F 
4 
P4 
F 
5 
P5 
F 
6 
P6 
F 
7 
P7 
F 
7 
P7 
F 
8 
P8 
F 
8 
P8 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
MT 
LMC 
NHV 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
User material type (41 - 50 inclusive).  A number between 41 and 
50  has  to  be  chosen.    If  MT < 0,  subroutine  rwumat  in  dyn21.f  is 
called, where the material parameter reading can be modified. 
WARNING:  If  two  or  more  materials  in  an  input 
deck share the same MT value, those materials also 
share  values  of  other  variables  on  Cards  1  and  2 
excluding  MID  and  RO.    Those  shared  values  are 
taken from the first material where the common MT 
is encountered. 
Length of material constant array which is equal to the number of 
material constants to be input.   
Number of history variables to be stored, see Appendix A.  When
the model is to be used with an equation of  state, NHV must be
increased by 4 to allocate the storage required by the equation of
state.
VARIABLE   
IORTHO/ 
ISPOT 
DESCRIPTION
EQ.1: if the material is orthotropic. 
EQ.2: if material is used with spot weld thinning. 
EQ.3: if  material  is  orthotropic  and  used  with  spot  weld
thinning 
IBULK 
IG 
IVECT 
Address  of  bulk  modulus  in  material  constants  array,  see
Appendix A. 
Address  of  shear  modulus  in  material  constants  array,  see
Appendix A. 
Vectorization flag (on = 1).  A vectorized user subroutine must be 
supplied. 
IFAIL 
Failure flag. 
EQ.0: No failure, 
EQ.1: Allows failure of shell and solid elements, 
LT.0:  |IFAIL|  is  the  address  of  NUMINT  in  the  material
constants  array.    NUMINT  is  defined  as  the  number  of
failed  integration  points  that  will  trigger  element  dele-
tion.  This option applies only to shell and solid elements
(release 5 of version 971). 
ITHERM 
Temperature flag (on = 1).  Compute element temperature. 
IHYPER 
Deformation  gradient  flag  (on = 1  or  –1,  or  3).    Compute  defor-
mation gradient, see Appendix A. 
IEOS 
Equation of state (on = 1). 
LMCA 
Length of additional material constant array. 
AOPT 
Material  axes  option  : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES, and then, for shells only, rotated about
the shell element normal by an angle BETA. 
EQ.1.0: locally orthotropic with material axes determined by a
point  in  space  and  the  global  location  of  the  element
center;  this  is  the  𝑎-direction.    This  option  is  for  solid
VARIABLE   
DESCRIPTION
elements only. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by 
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element 
defined  by  the  cross  product  of  the  vector  𝐯  with  the 
element normal. 
EQ.4.0: locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector 𝐯,  and 
an originating point, 𝐩, which define the centerline ax-
is.  This option is for solid elements only. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM 
*DEFINE_
COORDINATE_VECTOR).  Available in R3 version of 
971 and later. 
or 
MACF 
Material axes change flag for brick elements for quick changes: 
EQ.1: No change, default, 
EQ.2: switch material axes 𝑎 and 𝑏, 
EQ.3: switch material axes 𝑎 and 𝑐, 
EQ.4: switch material axes 𝑏 and 𝑐. 
XP, YP, ZP 
Coordinates of point 𝐩 for AOPT = 1 and 4. 
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3 and 4. 
D1, D2, D3 
Components of vector 𝐝 for AOPT = 2. 
BETA 
IEVTS 
Material  angle  in  degrees  for  AOPT = 0  (shells  only)  and 
AOPT = 3.      BETA  may  be  overridden  on  the  element  card,  see
*ELEMENT_SHELL_BETA and *ELEMENT_SOLID_ORTHO.  
Address of 𝐸𝑎 for orthotropic material in thick shell formulation 5
. 
P1 
First material parameter.
VARIABLE   
DESCRIPTION
P2 
P3 
P4 
⋮ 
Second material parameter. 
Third material parameter. 
Fourth material parameter. 
⋮ 
PLMC 
LMCth material parameter. 
Remarks: 
1.  Cohesive Elements.  Material models for the cohesive element (solid element 
type 19) uses the first two material parameters to set flags in the element formula-
tion. 
a)  P1.    The  P1  field  controls  how  the  density  is  used  to  calculate  the  mass 
when determining the tractions at mid-surface (tractions are calculated on 
a surface midway between the surfaces defined by nodes 1-2-3-4 and 5-6-
7-8).  If P1 is set to 1.0, then the density is per unit area of the midsurface 
instead  of  per  unit  volume.    Note  that  the  cohesive  element  formulation 
permits the element to have zero or negative volume. 
b)  P2.  The second parameter, P2, specifies the number of integration points 
(one  to  four)  that  are required  to  fail  for the  element  to  fail.   If  it  is  zero, 
the element will not fail regardless of IFAIL.  The recommended value for 
P2 is 1. 
c)  Other Parameters.  The cohesive element only uses MID, RO, MT, LMC, 
NHV, IFAIL and IVECT in addition to the material parameters. 
d)  Appendix R.  See Appendix R for the specifics of the umat subroutine re-
quirements for the cohesive element. 
2.  Material Constants.  If IORTHO = 0, LMC must be ≤ 48.  If IORTHO = 1, LMC 
must  be  ≤  40.    If  more  material  constants  are  needed,  LMCA  may  be  used  to 
create  an  additional  material  constant  array.    There  is  no  limit  on  the  size  of 
LMCA. 
3.  Spot  weld  thinning.    If  the  user-defined  material  is  used  for  beam  or  brick 
element spot welds that are tied to shell elements, and SPOTHIN > 0 on *CON-
TROL_CONTACT,  then  spot  weld  thinning will  be  done  for those  shells  if  IS-
POT = 2.  Otherwise, it will not be done.
4.  Thick Shell Formulation 5.  IEVTS is optional and is used only by thick shell 
formulation  5.    It  points  to  the  position  of  𝐸𝑎  in  the  material  constants  array.  
Following 𝐸𝑎, the next 5 material constants must be 𝐸𝑏, 𝐸𝑐, 𝜈𝑏𝑎, 𝜈𝑐𝑎, and 𝜈𝑐𝑏.  This 
data enables thick shell formulation 5 to calculate an accurate thickness strain, 
otherwise the thickness strain will be based on the elastic constants pointed to 
by IBULK and IG.
*MAT_BAMMAN 
This  is  Material  Type  51.    It  allows  the  modeling  of  temperature  and  rate  dependent 
plasticity with a fairly complex model that has many input parameters [Bamman 1989]. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
  Card 2 
Variable 
1 
C1 
Type 
F 
  Card 3 
Variable 
1 
C9 
Type 
F 
  Card 4 
1 
2 
C2 
F 
2 
F 
2 
Variable 
C17 
C18 
Type 
F 
F 
3 
E 
F 
3 
C3 
F 
3 
4 
PR 
F 
4 
C4 
F 
4 
5 
T 
F 
5 
C5 
F 
5 
6 
HC 
F 
6 
C6 
F 
6 
7 
8 
7 
C7 
F 
7 
8 
C8 
F 
8 
C10 
C11 
C12 
C13 
C14 
C15 
C16 
F 
F 
F 
F 
F 
3 
A1 
F 
4 
A2 
F 
5 
A4 
F 
6 
A5 
F 
7 
A6 
F 
F 
8 
KAPPA 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus (psi)
VARIABLE   
DESCRIPTION
PR 
T 
HC 
C1 
C2 
C3 
C4 
C5 
C6 
C7 
C8 
C9 
C10 
C11 
C12 
C13 
C14 
C15 
C16 
C17 
C18 
A1 
A2 
Poisson’s ratio 
Initial temperature (°R, degrees Rankine) 
Heat generation coefficient (°R⁄psi) 
Psi 
°R 
Psi 
°R 
1/s 
°R 
1/psi 
°R 
Psi 
°R 
1/psi-s 
°R 
1/psi 
°R 
psi 
°R 
1/psi-s 
°R 
α1, initial value of internal state variable 1 
α2, initial value of internal state variable 2.  Note:  α3 = -(α1 + α2 )
VARIABLE   
A3 
A4 
A5 
DESCRIPTION
α4, initial value of internal state variable 3 
α5, initial value of internal state variable 4 
α6, initial value of internal state variable 5 
KAPPA 
κ, initial value of internal state variable 6 
Unit Conversion Table 
Sec × psi × oR 
C1 
C2 
C3 
C4 
C5 
C6 
C7 
C8 
C9 
C10 
C11 
C12 
C13 
C14 
C15 
C16 
C17 
C18 
C0 = HC 
E 
 
T 
sec × MPa × oR 
×  1⁄145 
  — 
×  1⁄145 
  — 
  — 
  — 
×  145 
  — 
×  1⁄145 
  — 
×  145 
  — 
×  145 
  — 
×  1⁄145 
  — 
×  145 
  — 
×  145 
×  1⁄145 
— 
  — 
sec × MPA × oK 
×  1⁄145 
×  5⁄9 
×  1⁄145 
×  5⁄9 
  — 
×  5/9 
×  145 
×  5⁄9 
×  1⁄145 
×  5⁄9 
×  145 
×  5⁄9 
×  145 
×  5⁄9 
×  1⁄145 
×  5⁄9 
×  145 
×  5⁄9 
×  (145)(5⁄9) 
×  1⁄145 
  — 
×  5⁄9
*MAT_051 
The  kinematics  associated  with  the  model  are  discussed  in  references  [Hill  1948, 
Bammann  and  Aifantis  1987,  Bammann  1989].    The  description  below  is  taken  nearly 
verbatim from Bammann [1989]. 
With the assumption of linear elasticity we can write, 
where the Cauchy stress σ is convected with the elastic spin 𝑾 𝑒 as, 
= 𝜆 tr(𝑫𝑒)𝟏 + 2𝜇𝑫𝑒 
= 𝝈̇ − 𝑾 𝑒𝝈 + 𝝈𝑾 𝑒 
This  is  equivalent  to  writing  the  constitutive  model  with  respect  to  a  set  of  directors 
whose  direction  is  defined  by  the  plastic  deformation  [Bammann  and  Aifantis  1987, 
Bammann and Johnson 1987].  Decomposing both the skew symmetric and symmetric 
parts  of  the  velocity  gradient  into  elastic  and  plastic  parts  we  write  for  the  elastic 
stretching 𝑫𝑒 and the elastic spin 𝑾 𝑒, 
𝑫𝑒 = 𝑫 − 𝑫𝑝 − 𝑫𝑡ℎ, 𝑾 𝑒 = 𝑾 = 𝑾 𝑝. 
Within this structure it is now necessary to prescribe an equation for the plastic spin 𝑾 𝑝 
in  addition  to  the  normally  prescribed  flow  rule  for  𝑫𝑝  and  the  stretching  due  to  the 
thermal expansion 𝐷𝑡ℎ. As proposed, we assume a flow rule of the form, 
𝑫𝑝 = 𝑓 (𝑇)sinh [
|𝜉 | − 𝜅 − 𝑌(𝑇)
𝑉(𝑇)
]
𝝃′
∣𝜉′∣
. 
where  T  is  the  temperature,  κ  is  the  scalar  hardening  variable,  and  ξ′  is  the  difference 
between the deviatoric Cauchy stress σ′ and the tensor variable α′, 
𝝃′ = 𝝈′ − 𝜶′ 
and  f(T),  Y(T),  V(T)  are    scalar  functions  whose  specific  dependence  upon  the 
temperature  is  given  below.    Assuming  isotropic  thermal  expansion  and  introducing 
the expansion coefficient Ȧ , the thermal stretching can be written, 
𝑫𝑡ℎ = 𝐴̇𝑇̇𝟏 
The  evolution  of  the  internal  variables  α  and  κ  are  prescribed  in  a  hardening  minus 
recovery format as, 
⋅
= ℎ(𝑇)𝑫𝑝 − [𝑟𝑑(𝑇)|𝑫𝑝| + 𝑟𝑠(𝑇)]|𝜶|𝜶, 
= 𝐻(𝑇)𝑫𝑝 − [𝑅𝑑(𝑇)|𝑫𝑝| + 𝑅𝑠(𝑇)]𝜿2 
where h and H are the hardening moduli, rs(T) and Rs(T) are scalar functions describing 
the  diffusion  controlled  ‘static’  or  ‘thermal’  recovery,  and  rd(T)  and  Rd(T)  are  the 
functions describing dynamic recovery.
If  we  assume  that  Wp = 0,  we  recover  the  Jaumann  stress  rate  which  results  in  the 
prediction of an oscillatory shear stress response in simple shear when coupled with a 
Prager  kinematic  hardening  assumption  [Johnson  and  Bammann  1984].    Alternatively 
we can choose, 
𝑾 𝑝 = 𝑹𝑇𝑼̇ 𝑼 −1𝑹, 
which  recovers  the  Green-Naghdi  rate  of  Cauchy  stress  and  has  been  shown  to  be 
equivalent  to  Mandel’s  isoclinic  state  [Bammann  and  Aifantis  1987].    The  model 
employing  this  rate  allows  a  reasonable  prediction  of  directional  softening  for  some 
materials,  but  in  general  under-predicts  the  softening  and  does  not  accurately  predict 
the axial stresses which occur in the torsion of the thin walled tube. 
The final equation necessary to complete our description of high strain rate deformation 
is one which allows us to compute the temperature change during the deformation.  In 
the  absence  of  a  coupled  thermo-mechanical  finite  element  code  we  assume  adiabatic 
temperature  change  and  follow  the  empirical  assumption  that  90  -95%  of  the  plastic 
work is dissipated as heat.  Hence, 
𝑇̇ =
. 9
𝜌𝐶𝑣
(𝝈 ⋅ 𝑫𝑝), 
where ρ is the density of the material and Cv the specific heat. 
In terms of the input parameters the functions defined above become: 
  V(T)   =   C1 exp(-C2/T) 
h(T)   =   C9 exp(C10/T) 
  Y(T)   =   C3 exp(C4/T) 
rs(T)   =   C11exp(-C12/T) 
f(T)   =   C5 exp(-C6/T) 
  RD(T)   =   C13exp(-C14/T) 
rd(T)   =   C7 exp(-C8/T) 
  H(T)   =   C15exp(C16/T) 
  RS(T)   =   C17exp(-C18/T) 
and the heat generation coefficient is 
𝐻𝐶 =
0.9
𝜌𝐶𝑣
.
*MAT_052 
This is Material Type 52.  This is an extension of model 51 which includes the modeling 
of damage.  See Bamman et al.  [1990]. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
  Card 2 
Variable 
1 
C1 
Type 
F 
  Card 3 
Variable 
1 
C9 
Type 
F 
  Card 4 
1 
2 
C2 
F 
2 
F 
2 
Variable 
C17 
C18 
Type 
F 
F 
  Card 5 
Variable 
Type 
1 
N 
F 
2 
D0 
F 
3 
E 
F 
3 
C3 
F 
3 
4 
PR 
F 
4 
C4 
F 
4 
5 
T 
F 
5 
C5 
F 
5 
6 
HC 
F 
6 
C6 
F 
6 
7 
8 
7 
C7 
F 
7 
8 
C8 
F 
8 
F 
F 
F 
F 
F 
F 
4 
A2 
F 
4 
5 
A3 
F 
5 
6 
A4 
F 
6 
7 
A5 
F 
7 
8 
A6 
F 
8 
3 
A1 
F 
3 
FS 
F 
C10 
C11 
C12 
C13 
C14 
C15 
C16
MID 
*MAT_BAMMAN_DAMAGE 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
E 
PR 
T 
HC 
C1 
C2 
C3 
C4 
C5 
C6 
C7 
C8 
C9 
C10 
C11 
C12 
C13 
C14 
C15 
C16 
Mass density 
Young’s modulus (psi) 
Poisson’s ratio 
Initial temperature (°R, degrees Rankine) 
Heat generation coefficient (°R⁄psi) 
Psi 
°R 
Psi 
°R 
1/s 
°R 
1/psi 
°R 
Psi 
oR 
1/psi-s 
°R 
1/psi 
°R 
psi 
°R
VARIABLE   
DESCRIPTION
C17 
C18 
A1 
A2 
A3 
A4 
A5 
A6 
N 
D0 
FS 
1/psi-s 
°R 
1, initial value of internal state variable 1 
2, initial value of internal state variable 2 
3, initial value of internal state variable 3 
4, initial value of internal state variable 4 
α5, initial value of internal state variable 5 
α6, initial value of internal state variable 6 
Exponent in damage evolution 
Initial damage (porosity) 
Failure strain for erosion. 
Remarks: 
The evolution of the damage parameter, φ is defined by Bammann et al.  [1990] 
in which 
𝜙̇ = 𝛽 [
(1 − 𝜙)𝑁 − (1 − 𝜙)]
∣𝑫𝑝∣
𝛽 = sinh [
2(2𝑁 − 1)𝑝
(2𝑁 − 1)𝜎̅̅̅̅̅
] 
where p is the pressure and 𝜎̅̅̅̅̅ is the effective stress.
*MAT_CLOSED_CELL_FOAM 
This  is  Material  Type  53.    This  allows  the  modeling  of  low  density,  closed  cell 
polyurethane foam.  It is for simulating impact limiters in automotive applications.  The 
effect of the confined air pressure is included with the air being treated as an ideal gas.  
The general behavior is isotropic with uncoupled components of the stress tensor. 
3 
E 
F 
3 
4 
A 
F 
4 
5 
B 
F 
5 
6 
C 
F 
6 
7 
P0 
F 
7 
8 
PHI 
F 
8 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
Variable 
GAMA0 
LCID 
Type 
F 
I 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density 
E 
A 
B 
C 
P0 
PHI 
Young’s modulus 
a, factor for yield stress definition, see notes below. 
b, factor for yield stress definition, see notes below. 
c, factor for yield stress definition, see notes below. 
Initial foam pressure, P0 
Ratio of foam to polymer density, φ 
GAMA0 
Initial volumetric strain, γ0.  The default is zero.
DESCRIPTION
Optional  load  curve  defining  the  von  Mises  yield  stress  versus
−𝛾.  If the load curve ID is given, the yield stress is taken from the
curve  and  the  constants  a,  b,  and  c  are  not  needed.    The  load
curve is defined in the positive quadrant, i.e., positive values of 𝛾
are defined as negative values on the abscissa. 
  VARIABLE   
LCID 
Remarks: 
A  rigid,  low  density,  closed  cell,  polyurethane  foam  model  developed  at  Sandia 
Laboratories  [Neilsen,  Morgan  and  Krieg  1987]  has  been  recently  implemented  for 
modeling  impact  limiters  in  automotive  applications.    A  number  of  such  foams  were 
tested at Sandia and reasonable fits to the experimental data were obtained. 
In some respects this model is similar to the crushable honeycomb model type 26 in that 
the  components  of  the  stress  tensor  are  uncoupled  until  full  volumetric  compaction  is 
achieved. 
  However,  unlike  the  honeycomb  model  this  material  possesses  no 
directionality  but  includes  the  effects  of  confined  air  pressure  in  its  overall  response 
characteristics. 
𝜎𝑖𝑗 = 𝜎𝑖𝑗
sk − 𝛿𝑖𝑗𝜎 air 
where 𝜎𝑖𝑗
𝑠𝑘 is the skeletal stress and 𝜎 𝑎𝑖𝑟 is the air pressure computed from the equation: 
𝜎 air = −
𝑝0𝛾
1 + 𝛾 − 𝜙
where p0 is the initial foam pressure, usually taken as the atmospheric pressure, and γ 
defines the volumetric strain  
𝛾 = 𝑉 − 1 + 𝛾0 
where V is the relative volume, defined as the ratio of the current volume to the initial 
volume,  and  γ0  is  the  initial  volumetric  strain,  which  is  typically  zero.    The  yield 
condition is applied to the principal skeletal stresses, which are updated independently 
of the air pressure.  We first obtain the skeletal stresses: 
and compute the trial stress, σskt 
𝜎𝑖𝑗
sk = 𝜎𝑖𝑗 + 𝜎𝑖𝑗𝜎 air 
skt   = 𝜎𝑖𝑗
𝜎𝑖𝑗
sk + 𝐸 𝜀̇𝑖𝑗 Δ𝑡 
where  E  is  Young’s  modulus.    Since  Poisson’s  ratio  is  zero,  the  update  of  each  stress 
component is uncoupled and 2G = E where G is the shear modulus.  The yield condition 
is applied to the principal skeletal stresses such that, if the magnitude of a principal trial 
stress component, 𝜎𝑖
𝑠𝑘𝑡, exceeds the yield stress, σ
y, then
sk = min(𝜎𝑦, ∣𝜎𝑖
𝜎𝑖
skt∣)
skt
skt∣
𝜎𝑖
∣𝜎𝑖
The yield stress is defined by 
𝜎𝑦 = 𝑎 + 𝑏(1 + 𝑐𝛾) 
where  a,  b,  and  c  are  user  defined  input  constants  and  γ  is  the  volumetric  strain  as 
defined  above.    After  scaling  the  principal  stresses  they  are  transformed  back  into  the 
global system and the final stress state is computed 
𝜎𝑖𝑗 = 𝜎𝑖𝑗
sk − 𝛿𝑖𝑗𝜎 air.
*MAT_ENHANCED_COMPOSITE_DAMAGE 
These are Material Types 54 - 55 which are  enhanced versions of the composite model 
material  type  22.    Arbitrary  orthotropic  materials,  e.g.,  unidirectional  layers  in 
composite  shell  structures  can  be  defined.    Optionally,  various  types  of  failure  can  be 
specified following either the suggestions of [Chang and Chang 1987b] or [Tsai and Wu 
1971].    In  addition  special  measures  are  taken  for  failure  under  compression.    See 
[Matzenmiller and Schweizerhof 1991]. 
By  using  the  user  defined 
integration  rule,  see  *INTEGRATION_SHELL,  the 
constitutive  constants  can  vary  through  the  shell  thickness.    For  all  shells,  except  the 
DKT  formulation,  laminated  shell  theory  can  be  activated  to  properly  model  the 
transverse  shear  deformation.    Lamination  theory  is  applied  to  correct  for  the 
assumption of a uniform constant shear strain through the thickness of the shell. 
For  sandwich  shells  where  the  outer  layers  are  much  stiffer  than  the  inner  layers,  the 
response  will  tend  to  be  too  stiff  unless  lamination  theory  is  used.    To  turn  on 
lamination theory see *CONTROL_SHELL.  A damage model for transverse shear strain 
to model interlaminar shear failure is available.  The definition of minimum stress limits 
is available for thin/thick shells and solids. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
EA 
F 
3 
4 
EB 
F 
4 
5 
EC 
F 
5 
Variable 
GAB 
GBC 
GCA 
(KF) 
AOPT 
2WAY 
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
Variable 
Type 
F 
F 
4 
A1 
F 
5 
A2 
F 
6 
7 
8 
PRBA 
PRCA 
PRCB 
F 
6 
F 
6 
F 
7 
TI 
F 
7 
F 
8 
8 
A3 
MANGLE 
F
Card 4 
Variable 
1 
V1 
Type 
F 
  Card 5 
1 
2 
V2 
F 
2 
3 
V3 
F 
3 
4 
D1 
F 
4 
5 
D2 
F 
5 
6 
7 
8 
D3 
DFAILM 
DFAILS 
F 
6 
F 
7 
F 
8 
Variable 
TFAIL 
ALPH 
SOFT 
FBRT 
YCFAC 
DFAILT 
DFAILC 
EFS 
Type 
F 
F 
F 
F 
F 
  Card 6 
Variable 
1 
XC 
Type 
F 
2 
XT 
F 
3 
YC 
F 
4 
YT 
F 
5 
SC 
F 
F 
6 
F 
7 
F 
8 
CRIT 
BETA 
F 
F 
Optional Card 7 (only for CRIT = 54) 
  Card 7 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PFL 
EPSF 
EPSR 
TSMD 
SOFT2 
Type 
F 
F 
F 
F 
F 
Optional Card 8 (only for CRIT = 54) 
  Card 8 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SLIMT1 
SLIMC1 
SLIMT2 
SLIMC2 
SLIMS 
NCYRED 
SOFTG 
Type 
F 
F 
F 
F 
F 
F
Optional Card 9 (only for CRIT = 54)  
  Card 9 
1 
2 
3 
4 
5 
Variable 
LCXC 
LCXT 
LCYC 
LCYT 
LCSC 
Type 
I 
I 
I 
I 
I 
7 
8 
6 
DT 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
EA 
EB 
EC 
PRBA 
PRCA 
PRCB 
GAB 
GBC 
GCA 
(KF) 
AOPT 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
𝐸𝑎, Young’s modulus - longitudinal direction 
𝐸𝑏, Young’s modulus - transverse direction 
𝐸𝑐, Young’s modulus - normal direction 
𝜈𝑏𝑎, Poisson’s ratio 𝑏𝑎 
𝜈𝑐𝑎, Poisson’s ratio 𝑐𝑎 
𝜈𝑐𝑏, Poisson’s ratio 𝑐𝑏 
𝐺𝑎𝑏, shear modulus 𝑎𝑏 
𝐺𝑏𝑐, shear modulus 𝑏𝑐 
𝐺𝑐𝑎, shear modulus 𝑐𝑎 
Bulk modulus of failed material (not used) 
Material  axes  option  : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES, and then, for shells only, rotated about 
the shell element normal by an angle MANGLE. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
VARIABLE   
DESCRIPTION
rotating the material axes about the element normal by 
an angle (MANGLE) from a line in the plane of the el-
ement defined by the cross product of the vector v with
the element normal. 
EQ.4.0: locally orthotropic in cylindrical coordinate system with
the  material  axes  determined  by  a  vector  𝐯,  and  an 
originating  point,  𝐩,  which  define  the  centerline  axis. 
This option is for solid elements only. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
2WAY 
Flag to turn on 2-way fiber action. 
EQ.0.0: Standard unidirectional behavior. 
EQ.1.0: 2-way  fiber  behavior.    The  meaning  of  the  fields
DFAILT,  DFAILC,  YC,  YT,  SLIMT2  and  SLIMC2  are 
altered  if  this  flag  is  set.    This  option  is  only  available
for MAT 54 using thin shells. 
TI 
Flag to turn on transversal isotropic behavior for MAT_054 solid
elements. 
EQ.0.0: Standard unidirectional behavior. 
EQ.1.0: transversal  isotropic  behavior  .  
A1, A2, A3 
Define components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
Define components of vector 𝐯 for AOPT = 3. 
D1, D2, D3 
Define components of vector 𝐝 for AOPT = 2. 
MANGLE 
Material  angle  in  degrees  for  AOPT = 0  (shells  only)  and 
AOPT = 3.      MANGLE  may  be  overridden  on  the  element  card,
see *ELEMENT_SHELL_BETA and *ELEMENT_SOLID_ORTHO.
VARIABLE   
DFAILM 
DESCRIPTION
Maximum  strain  for  matrix  straining  in  tension  or  compression
(active  only  for MAT_054  and  only  if  DFAILT > 0).    The  layer  in 
the  element  is  completely  removed  after  the  maximum  strain  in
the  matrix  direction  is  reached.    The  input  value  is  always
positive. 
DFAILS 
Maximum  tensorial  shear  strain  (active  only  for  MAT_054  and 
only  if  DFAILT > 0).    The  layer  in  the  element  is  completely
removed  after  the  maximum  shear  strain  is  reached.    The  input
value is always positive. 
TFAIL 
Time step size criteria for element deletion: 
tfail ≤ 0: 
no  element  deletion  by  time  step  size.    The
crashfront algorithm only works if tfail is set to a
value above zero. 
0 < tfail ≤ 0.1: element  is  deleted  when  its  time  step  is  smaller
than the given value, 
tfail > 0.1: 
element  is  deleted  when  the  quotient  of  the 
actual time step and the original time step drops
below the given value. 
ALPH 
SOFT 
Shear stress parameter for the nonlinear term, see Material 22. 
Softening  reduction  factor  for  material  strength  in  crashfront
elements  (default = 1.0).    TFAIL  must  be  greater  than  zero  to 
activate this option. 
FBRT 
Softening for fiber tensile strength: 
EQ.0.0: tensile strength = XT 
GT.0.0:  tensile  strength = XT,  reduced  to  XT ×  FBRT  after 
failure has occurred in compressive matrix mode. 
YCFAC 
Reduction  factor  for  compressive  fiber  strength  after  matrix
compressive  failure  (MAT_054  only).    The  compressive  strength 
in  the  fiber  direction  after  compressive  matrix  failure  is  reduced
to: 
𝑋𝑐 = YCFAC × 𝑌𝑐,
(default: YCFAC = 2.0)
VARIABLE   
DFAILT 
DESCRIPTION
Maximum  strain  for  fiber  tension  (MAT_054  only).    (Maximum 
1 = 100% strain).  The layer in the element is completely removed
after the maximum tensile strain in the fiber direction is reached.
If a nonzero value is given for DFAILT, a nonzero, negative value
must also be provided for DFAILC. 
If  the  2-way  fiber  flag  is  set  then  DFAILT  is  the  fiber  tensile
failure strain in the 𝑎 and 𝑏 directions. 
DFAILC 
EFS 
XC 
XT 
YC 
for 
fiber  compression 
(MAT_054  only). 
Maximum  strain 
(Maximum  -1 = 100%  compression).    The  layer  in  the  element  is 
completely removed after the maximum compressive strain in the
fiber  direction  is  reached.    The  input  value  should  be  negative
and is required if DFAILT > 0. 
If the 2-way fiber flag is set then DFAILC is the fiber compressive
failure strain in the 𝑎 and 𝑏 directions. 
Effective failure strain (MAT_054 only). 
Longitudinal compressive strength (absolute value is used). 
GE.0.0: Poisson effect (PRBA) after failure is active. 
LT.0.0:  Poisson effect after failure is not active, i.e.  PRBA = 0. 
Longitudinal tensile strength, see below. 
Transverse  compressive  strength,  𝑏-axis  (positive  value),  see 
below. 
If  the  2-way  fiber  flag  is  set  then  YC  is  the  fiber  compressive
failure stress in the 𝑏 direction. 
YT 
Transverse tensile strength, 𝑏-axis, see below. 
If  the  2-way  fiber  flag  is  set  then  YT  is  the  fiber  tensile  failure
stress in the 𝑏 direction. 
SC 
Shear strength, ab plane, see below.
VARIABLE   
DESCRIPTION
CRIT 
Failure criterion (material number): 
BETA 
PFL 
EPSF 
EPSR 
TSMD 
SOFT2 
SLIMT1 
SLIMC1 
SLIMT2 
EQ.54.0: Chang  criterion  for  matrix  failure  (as  Material  22) 
(default), 
EQ.55.0: Tsai-Wu criterion for matrix failure. 
Weighting  factor  for  shear  term  in  tensile  fiber  mode  (MAT_054 
only).  (0.0 ≤ BETA ≤ 1.0) 
Percentage  of  layers  which  must  fail  until  crashfront  is  initiated.
E.g.  |PFL| = 80.0,  then  80%  of  layers  must  fail  until  strengths  are 
reduced in neighboring elements.  Default: all layers must fail.  A
single layer fails if 1 in-plane IP fails (PFL > 0) or if 4 in-plane IPs 
fail (PFL < 0).  (MAT_054 only, thin and thick shells). 
Damage initiation transverse shear strain.  (MAT_054 only). 
Final rupture transverse shear strain.  (MAT_054 only). 
Transverse  shear  maximum  damage,  default = 0.90.    (MAT_054 
only,). 
Optional  “orthogonal”  softening  reduction  factor  for  material
strength  in  crashfront  elements  (default = 1.0).    See  remarks 
(MAT_054 only, thin and thick shells). 
Factor  to  determine  the  minimum  stress  limit  after  stress
maximum (fiber tension).  Similar to *MAT_058 (MAT_054 only).
Factor  to  determine  the  minimum  stress  limit  after  stress
maximum  (fiber  compression).    Similar  to  *MAT_058  (MAT_054 
only). 
Factor  to  determine  the  minimum  stress  limit  after  stress
maximum  (matrix  tension).    Similar  to  *MAT_058  (MAT_054 
only). 
If the 2-way fiber flag is set then SLIMT2 is the factor to determine
the  minimum  stress  limit  after  tensile  failure  stress  is  reached  in
the 𝑏 fiber direction.
VARIABLE   
SLIMC2 
SLIMS 
NCYRED 
SOFTG 
LCXC 
LCXT 
LCYC 
LCYT 
LCSC 
DESCRIPTION
Factor  to  determine  the  minimum  stress  limit  after  stress
maximum (matrix compression).  Similar to *MAT_058 (MAT_054 
only). 
If  the  2-way  fiber  flag  is  set  then  SLIMC2  is  the  factor  to
determine  the  minimum  stress  limit  after  compressive  failure
stress is reached in the 𝑏 fiber direction. 
Factor  to  determine  the  minimum  stress  limit  after  stress
maximum (shear).  Similar to *MAT_058 (MAT_054 only). 
Number  of  cycles  for  stress  reduction  from  maximum  to
minimum (MAT_054 only). 
Softening  reduction  factor  for  transverse  shear  moduli  GBC  and
GCA  in  crashfront  elements  (default = 1.0)  (MAT_054  only,  thin 
and thick shells). 
Load  curve  ID  for  XC  vs.    strain  rate  (XC  is  ignored  with  that
option) 
Load  curve  ID  for  XT  vs.    strain  rate  (XT  is  ignored  with  that
option) 
Load  curve  ID  for  YC  vs.    strain  rate  (YC  is  ignored  with  that
option) 
Load  curve  ID  for  YT  vs.    strain  rate  (YT  is  ignored  with  that
option) 
Load  curve  ID  for  SC  vs.    strain  rate  (SC  is  ignored  with  that 
option) 
DT 
Strain rate averaging option. 
EQ.0.0: Strain rate is evaluated using a running average. 
LT.0.0:  Strain  rate  is  evaluated  using  average  of  last  11  time
steps. 
GT.0.0:  Strain rate is averaged over the last DT time units. 
Material Formulation: 
The Chang/Chang (MAT_54) criteria is given as follows:
for the tensile fiber mode, 
𝜎𝑎𝑎 > 0 ⇒ 𝑒𝑓
2 = (
)
𝜎𝑎𝑎
𝑋𝑡
+ 𝛽 (
𝜎𝑎𝑏
𝑆𝑐
)
− 1,
2 ≥ 0 ⇒ failed 
𝑒𝑓
2 < 0 ⇒ elastic
𝑒𝑓
𝐸𝑎 = 𝐸𝑏 = 𝐺𝑎𝑏 = 𝜈𝑏𝑎 = 𝜈𝑎𝑏 = 0 
for the compressive fiber mode, 
𝜎𝑎𝑎 < 0 ⇒ 𝑒𝑐
2 = (
− 1,
)
𝜎𝑎𝑎
𝑋𝑐
2 ≥ 0 ⇒ failed 
𝑒𝑐
2 < 0 ⇒ elastic
𝑒𝑐
𝐸𝑎 = 𝜈𝑏𝑎 = 𝜈𝑎𝑏 = 0 
for the tensile matrix mode, 
𝜎𝑏𝑏 > 0 ⇒ 𝑒𝑚
2 = (
𝜎𝑏𝑏
𝑌𝑡
)
+ (
𝜎𝑎𝑏
𝑆𝑐
)
− 1,
2 ≥ 0 ⇒ failed 
𝑒𝑚
2 < 0 ⇒ elastic
𝑒𝑚
𝐸𝑏 = 𝜈𝑏𝑎 = 0 ⇒ 𝐺𝑎𝑏 = 0, 
and for the compressive matrix mode, 
𝜎𝑏𝑏 < 0 ⇒ 𝑒𝑑
2 = (
𝜎𝑏𝑏
2𝑆𝑐
)
+
)
𝑌𝑐
2𝑆𝑐
⎢⎡(
⎣
− 1
⎥⎤ 𝜎𝑏𝑏
𝑌𝑐
⎦
+ (
)
𝜎𝑎𝑏
𝑆𝑐
− 1,
2 ≥ 0 ⇒ failed 
𝑒𝑑
2 < 0 ⇒ elastic
𝑒𝑑
𝐸𝑏 = 𝜈𝑏𝑎 = 𝜈𝑎𝑏 = 0 ⇒ 𝐺𝑎𝑏 = 0 
𝑋𝑐 = 2𝑌𝑐, for 50% fiber volume 
If  the  2-way  fiber  flag  is  set  then  the  failure  criteria  for  tensile  and  compressive  fiber 
failure in the local X direction are unchanged.  For the local 𝑦-direction, the same failure 
criteria as for the 𝑥-direction fibers are used. 
Tension, 𝑦-direction, 
𝜎𝑏𝑏 > 0 ⇒ 𝑒𝑓
2 = (
)
𝜎𝑏𝑏
𝑌𝑡
+ 𝛽 (
𝜎𝑎𝑏
𝑆𝑐
) − 1,
2 ≥ 0 ⇒ failed 
𝑒𝑓
2 < 0 ⇒ elastic
𝑒𝑓
Compressive 𝑦-direction, 
𝜎𝑏𝑏 < 0 ⇒ 𝑒𝑐
2 = (
𝜎𝑏𝑏
𝑌𝑐
)
− 1,
2 ≥ 0 ⇒ failed 
𝑒𝑐
2 < 0 ⇒ elastic
𝑒𝑐
Matrix failure criterion,
2 = (
𝑒𝑓
)
𝜎𝑎𝑏
𝑆𝑐
− 1  
In the Tsai-Wu (MAT_055) criteria the tensile and compressive fiber modes are treated 
as  in  the  Chang-Chang  criteria.    The  failure  criterion  for  the  tensile  and  compressive 
matrix mode is given as: 
2 =
𝑒md
𝜎𝑏𝑏
𝑌𝑐𝑌𝑡
+ (
)
𝜎𝑎𝑏
𝑆𝑐
+
(𝑌𝑐 − 𝑌𝑡) 𝜎𝑏𝑏
𝑌𝑐𝑌𝑡
− 1,
2 ≥ 0 ⇒ failed 
𝑒𝑚𝑑
2 < 0 ⇒ elastic
𝑒𝑚𝑑
For  β = 1  we  get  the  original  criterion  of  Hashin  [1980]  in  the  tensile  fiber  mode.    For 
β = 0  we  get  the  maximum  stress  criterion  which  is  found  to  compare  better  to 
experiments. 
In MAT_054, failure can occur in any of four different ways: 
1. 
2. 
3. 
4. 
If DFAILT is zero, failure occurs if the Chang-Chang failure criterion is satisfied 
in the tensile fiber mode. 
If DFAILT is greater than zero, failure occurs if: 
- 
- 
- 
the fiber strain is greater than DFAILT or less than DFAILC 
if absolute value of matrix strain is greater than DFAILM 
if absolute value of tensorial shear strain is greater than DFAILS 
If  EFS  is  greater  than  zero,  failure  occurs  if  the  effective  strain  is  greater  than 
EFS. 
If TFAIL is greater than zero, failure occurs  according to the element timestep 
as described in the definition of TFAIL above. 
When  failure  has  occurred  in  all  the  composite  layers  (through-thickness  integration 
points), the element is deleted.  Elements  which  share nodes with the deleted element 
become “crashfront” elements and can have their strengths reduced by using the SOFT 
parameter with TFAIL greater than zero.  An earlier initiation of crashfront elements is 
possible by using parameter PFL.
Reduction 
by SOFT2 
(orthogonal
)
Reduction 
by 
0.5(SOFT+SOFT2) 
Reduction 
By SOFT (parallel) 
Figure M54-1.  Direction dependent softening 
An  optional  direction  dependent  strength  reduction  can  be  invoked  by  setting 
0 < SOFT2 < 1.    Then, SOFT  equals  a  strength  reduction  factor  for fiber  parallel  failure 
and  SOFT2  equals  a  strength  reduction  factor  for  fiber  orthogonal  failure.    Linear 
interpolation is used for angles in between.  See Figure M54-1. 
Information  about  the  status  in  each  layer  (integration  point)  and  element  can  be 
plotted  using  additional  integration  point  variables.    The  number  of  additional 
integration  point  variables  for  shells  written to the  LS-DYNA  database  is  input  by  the 
*DATABASE_EXTENT_BINARY  definition  as  variable  NEIPS.    For  Models  54  and  55 
these additional variables are tabulated below (i = shell integration point): 
History 
Variable 
1  ef(i) 
Description 
tensile fiber mode 
Value 
LS-PrePost 
History Variable
2  ec(i) 
compressive fiber mode 
3  em(i)  tensile matrix mode 
1  –   elastic 
4  ed(i) 
compressive 
mode 
5  efail  max[ef(ip)] 
matrix 
0  –  failed 
6  dam  damage parameter 
−1  –  element intact 
10−8 –  element 
crashfront 
+1  –  element failed 
in 
1 
2 
3 
4 
5 
6 
These  variables  can  be  plotted  in  LS-PrePost  element  history  variables  1  to  6.    The 
following  components,  defined  by  the  sum  of  failure  indicators  over  all  through-
thickness integration points, are stored as element component 7 instead of the effective 
plastic strain.
Description 
Integration point 
nip
nip
∑ 𝑒𝑓 (𝑖)
𝑖=1
nip
nip
∑ 𝑒𝑐(𝑖)
𝑖=1
nip
nip
∑ 𝑒𝑚(𝑖)
𝑖=1
1 
2 
3 
In  an  optional  damage  model  for  transverse  shear  strain,  out-of-plane  stiffness  (GBC 
and  GCA)  can  get  linearly  decreased  to  model  interlaminar  shear  failure.    Damage 
starts when effective transverse shear strain 
eff = √𝜀𝑦𝑧
𝜀56
2  
2 + 𝜀𝑧𝑥
reaches EPSF.  Final rupture occurs when effective transverse shear strain reaches EPSR.  
A  maximum  damage  of  TSMD  (0.0 < TSMD < 0.99)  cannot  be  exceeded.    See  Figure 
M54-2.
transverse shear stiffness 
transverse shear stiffness 
GBC, 
GBC, 
GCA 
GCA 
D=0 
D = 0 
D=TSMD 
D = TSMD 
EPSF 
EPSF 
EPSR
EPSR
transverse shear strain 
transverse shear strain 
Figure M54-3.  Linear Damage for transverse shear behavior 
Figure M54-2.  Linear Damage for transverse shear behavior 
Additional Remarks:  
1.  TI-Flag 
(Transversal isotropic behavior for *MAT_054 solid elements).   
The behavior in the b-c-plane is assumed to be isotropic, thus the elastic constants 
EC, PRCA and GCA are ignored and set according to the given values EA, EB, 
PRAB, GAB.  Damage in transverse shear (EPSF, EPSR, TSMD, SOFTG) is ignored.  
The failure criterion is evaluated by replacing  𝜎bb and 𝜎ab with the corresponding 
stresses  𝜎11 and 𝜎a1  in a principal stress frame rotated around the local a-axis.  
The principal axes 1 and 2 in the b-c plane are chosen such that |𝜎11| ≥ |𝜎22| is 
fulfilled.
*MAT_LOW_DENSITY_FOAM 
This is Material Type 57 for modeling highly compressible low density foams.  Its main 
applications  are  for  seat  cushions  and  padding  on  the  Side  Impact  Dummies  (SID).  
Optionally,  a  tension  cut-off  failure  can  be  defined.    A  table  can  be  defined  if  thermal 
effects are considered in the nominal stress versus strain behavior.  Also, see the notes 
below. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
LCID 
F 
Default 
Remarks 
5 
TC 
F 
1020 
  Card 2 
1 
2 
3 
4 
5 
6 
HU 
F 
1. 
3 
6 
7 
8 
BETA 
DAMP 
F 
F 
0.05 
8 
1 
7 
Variable 
SHAPE 
FAIL 
BVFLAG 
ED 
BETA1 
KCON 
REF 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
1.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Remarks 
3 
2 
5 
5 
6 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s modulus used in tension.  For implicit problems E is set
to the initial slope of load curve LCID.
VARIABLE   
LCID 
TC 
HU 
BETA 
DAMP 
DESCRIPTION
Load  curve  or  table  ID,  see  *DEFINE_CURVE,  for  the  nominal 
stress versus strain curve definition.  If a table is used, a family of
curves  is  defined  each  corresponding  to  a  discrete  temperature,
see *DEFINE_TABLE. 
Cut-off for the nominal tensile stress τi  
Hysteretic  unloading  factor  between  0  and  1  (default = 1,  i.e.,  no 
energy dissipation), see also Figure M57-1. 
β, decay constant to model creep in unloading 
Viscous  coefficient  (.05 < recommended  value  <.50)  to  model 
damping effects. 
LT.0.0: |DAMP|  is  the  load  curve  ID,  which  defines  the
damping constant as a function of the maximum strain
in compression defined as: 
𝜀max = max(1 − 𝜆1, 1 − 𝜆2, 1. −𝜆3). 
In  tension,  the  damping  constant  is  set  to  the  value  corre-
sponding  to  the  strain  at  0.    The  abscissa  should  be  defined
from 0 to 1. 
SHAPE 
Shape  factor  for  unloading.    Active  for  nonzero  values  of  the
hysteretic  unloading  factor.    Values  less  than  one  reduces  the 
energy dissipation and greater than one increases dissipation, see
also Figure M57-1. 
FAIL 
Failure option after cutoff stress is reached: 
EQ.0.0: tensile stress remains at cut-off value, 
EQ.1.0: tensile stress is reset to zero. 
BVFLAG 
Bulk viscosity activation flag, see remark below: 
EQ.0.0: no bulk viscosity (recommended), 
EQ.1.0: bulk viscosity active. 
ED 
Optional  Young's  relaxation  modulus,  𝐸𝑑,  for  rate  effects.    See 
Remark 5. 
BETA1 
Optional decay constant, 𝛽1.
Typical unloading
curves determined by
the hysteretic unloading
factor. With the shape
factor equal to unity.
Typical unloading for
a large shape factor, e.g. 
5.0-8.0, and a small 
hystereticfactor, e.g., 0.010.
Unloading
curves
Strain
Strain
Figure M57-1.  Behavior of the low density urethane foam model 
  VARIABLE   
KCON 
DESCRIPTION
Stiffness  coefficient  for  contact  interface  stiffness.    If  undefined
the maximum slope in stress vs.  strain curve is used.  When the
maximum slope is taken for the contact, the time step size for this
material  is  reduced  for  stability.    In  some  cases  Δt  may  be 
significantly  smaller,  and  defining  a  reasonable  stiffness  is
recommended. 
REF 
Use  reference  geometry  to  initialize  the  stress  tensor.    The
reference geometry is defined by the keyword:*INITIAL_FOAM_-
REFERENCE_GEOMETRY . 
EQ.0.0: off, 
EQ.1.0: on. 
Material Formulation: 
The compressive behavior is illustrated in Figure M57-1 where hysteresis on unloading 
is shown.  This behavior under uniaxial loading is assumed not to significantly couple 
in  the  transverse  directions.    In  tension  the  material  behaves  in  a  linear  fashion  until 
tearing  occurs.    Although  our  implementation  may  be  somewhat  unusual,  it  was 
motivated by Storakers [1986]. 
The model uses tabulated input data for the loading curve where the nominal stresses 
are  defined  as  a  function  of  the  elongations,  𝜀𝑖,  which  are  defined  in  terms  of  the 
principal stretches, 𝜆𝑖, as: 
𝜀𝑖 = 𝜆𝑖 − 1 
The principal stretches are stored as extra history variables 16, 17, and 18 if ED = 0 and 
as  extra  history  variables  28,  29,  and  30  if  ED > 0.        The  stretch  ratios  are  found  by
solving for the eigenvalues of the left stretch tensor, 𝑉𝑖𝑗, which is obtained via a polar 
decomposition of the deformation gradient matrix, 𝐹𝑖𝑗.  Recall that,  
𝐹𝑖𝑗 = 𝑅𝑖𝑘𝑈𝑘𝑗 = 𝑉𝑖𝑘𝑅𝑘𝑗 
The  update  of  Vij  follows  the  numerically  stable  approach  of  Taylor  and  Flanagan 
[1989].  After solving for the principal stretches, we compute the elongations and, if the 
elongations  are  compressive,  the  corresponding  values  of  the  nominal  stresses,  𝜏𝑖  are 
interpolated.  If the elongations are tensile, the nominal stresses are given by 
and the Cauchy stresses in the principal system become 
𝜏𝑖 = 𝐸𝜀𝑖 
𝜎𝑖 =
𝜏𝑖
𝜆𝑗𝜆𝑘
The  stresses  can  now  be  transformed  back  into  the  global  system  for  the  nodal  force 
calculations. 
Remarks: 
1.  When  hysteretic  unloading  is  used  the  reloading  will  follow  the  unloading 
curve  if  the  decay  constant,  β,  is  set  to  zero.    If  β  is  nonzero  the  decay  to  the 
original loading curve is governed by the expression: 
1 − 𝑒−𝛽𝑡 
2.  The  bulk  viscosity,  which  generates  a  rate  dependent  pressure,  may  cause  an 
unexpected  volumetric  response  and,  consequently,  it  is  optional  with  this 
model. 
3.  The hysteretic unloading factor results in the unloading curve to lie beneath the 
loading curve as shown in Figure M57-1 This unloading provides energy dissi-
pation which is reasonable in certain kinds of foam. 
4.  Note that since this material has no effective plastic strain, the internal energy 
per initial volume is written into the output databases. 
5.  Rate  effects  are  accounted  for  through  linear  viscoelasticity  by  a  convolution 
integral of the form 
𝜎𝑖𝑗
𝑟 = ∫ 𝑔𝑖𝑗𝑘𝑙
(𝑡 − 𝜏)
∂𝜀𝑘𝑙
∂𝜏
𝑑𝜏 
where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) is the relaxation function.  The stress tensor, 𝜎𝑖𝑗
stresses  determined  from  the  foam,  𝜎𝑖𝑗
taken as the summation of the two contributions: 
𝑟 , augments the 
𝑓 ;  consequently,  the  final  stress,  𝜎𝑖𝑗,  is 
𝜎𝑖𝑗 = 𝜎𝑖𝑗
𝑓 + 𝜎𝑖𝑗
𝑟 .
Since  we  wish  to  include  only  simple  rate  effects,  the  relaxation  function  is 
represented by one term from the Prony series: 
given by, 
𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚
𝑚=1
𝑒−𝛽 𝑡 
𝑔(𝑡) = 𝐸𝑑𝑒−𝛽1 𝑡 
This model is effectively a Maxwell fluid which consists of a damper and spring 
in series.  We characterize this in the input by a Young's modulus, 𝐸𝑑, and de-
cay constant, 𝛽1.  The formulation is performed in the local system of principal 
stretches  where  only  the  principal  values  of  stress  are  computed  and  triaxial 
coupling  is  avoided.    Consequently,  the  one-dimensional  nature  of  this  foam 
material  is  unaffected  by  this  addition  of  rate  effects.    The  addition  of  rate  ef-
fects necessitates twelve additional history variables per integration point.  The 
cost  and  memory  overhead  of  this  model  comes  primarily  from  the  need  to 
“remember” the local system of principal stretches. 
6.  The  time  step  size  is  based  on  the  current  density  and  the  maximum  of  the 
instantaneous  loading  slope,  𝐸,  and  KCON.    If  KCON  is  undefined  the  maxi-
mum slope in the loading curve is used instead.
*MAT_LAMINATED_COMPOSITE_FABRIC 
This is Material Type 58.  Depending on the type of failure surface, this model may be 
used to model composite materials with unidirectional layers, complete laminates, and 
woven  fabrics.    This  model  is  implemented  for  shell  and  thick  shell  elements 
(ELFORM = 1 and 2). 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
EA 
F 
3 
4 
EB 
F 
4 
5 
6 
7 
8 
(EC) 
PRBA 
TAU1 
GAMMA1
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
GAB 
GBC 
GCA 
SLIMT1 
SLIMC1 
SLIMT2 
SLIMC2 
SLIMS 
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
F 
4 
Variable 
AOPT 
TSIZE 
ERODS 
SOFT 
Type 
F 
F 
F 
F 
  Card 4 
Variable 
1 
XP 
Type 
F 
  Card 5 
Variable 
1 
V1 
Type 
F 
LS-DYNA R10.0 
2 
YP 
F 
2 
V2 
F 
3 
ZP 
F 
3 
V3 
F 
4 
A1 
F 
4 
D1 
F 
F 
5 
FS 
F 
5 
A2 
F 
5 
D2 
F 
F 
6 
F 
7 
F 
8 
EPSF 
EPSR 
TSMD 
F 
6 
A3 
F 
6 
D3 
F 
F 
7 
F 
8 
PRCA 
PRCB 
F 
8 
F 
7 
BETA
Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
E11C 
E11T 
E22C 
E22T 
GMS 
Type 
F 
F 
F 
F 
F 
  Card 7 
Variable 
1 
XC 
Type 
F 
2 
XT 
F 
3 
YC 
F 
4 
YT 
F 
5 
SC 
F 
6 
7 
8 
First Optional Strain Rate Dependence Card. 
  Card 8 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCXC 
LCXT 
LCYC 
LCYT 
LCSC 
LCTAU 
LCGAM 
DT 
Type 
I 
I 
I 
I 
I 
I 
I 
F 
Second Optional Strain Rate Dependence Card. 
  Card 9 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCE11C 
LCE11T 
LCE22C 
LCE22T 
LCGMS 
LCEFS 
Type 
I 
I 
I 
I 
I 
I 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density
VARIABLE   
EA 
DESCRIPTION
GT.0.0:  𝐸𝑎, Young’s modulus - longitudinal direction 
LT.0.0:  Load curve ID or Table ID = (-EA) 
Load Curve. When (-EA) is equal to a Load curve ID, 
it  is  taken  as  defining  the  uniaxial  elastic  stress  vs.
strain behavior in longitudinal direction. 
Tabular  Data.  When  (-EA)  is  equal  to  a  Table  ID,  it 
defines for each strain rate value a Load curve ID giv-
ing  the  uniaxial  elastic  stress  vs.    strain  behavior  in
longitudinal direction. 
Logarithmically  Defined  Tables.  If  the  first  uniaxial 
elastic  stress  vs.    strain  curve  in  the  table  corresponds 
to  a  negative  strain  rate,  LS-DYNA  assumes  that  the 
natural logarithm of the strain rate value is used for all
stress-strain curves. 
EB 
GT.0.0:  𝐸𝑏, Young’s modulus - transverse direction 
LT.0.0:  Load curve ID or Table ID = (-EB) 
Load Curve. When (-EB) is equal to a Load curve ID, it 
is taken as defining the uniaxial elastic stress vs.  strain
behavior in transverse direction. 
Tabular  Data.  When  (-EB)  is  equal  to  a  Table  ID,  it 
defines for each strain rate value a Load curve ID giv-
ing  the  uniaxial  elastic  stress  vs.    strain  behavior  in 
transverse direction. 
Logarithmically  Defined  Tables.  If  the  first  uniaxial 
elastic  stress  vs.    strain  curve  in  the  table  corresponds
to  a  negative  strain  rate,  LS-DYNA  assumes  that  the 
natural logarithm of the strain rate value is used for all
stress-strain curves. 
(EC) 
PRBA 
PRCA 
PRCB 
Ec, Young’s modulus - normal direction (not used) 
𝜈𝑏𝑎, Poisson’s ratio ba 
𝜈𝑐𝑎,  Poisson’s  ratio  ca,  can  be  defined  in  card  4,  col.    7,
default = PRBA 
𝜈𝑐𝑏,  Poisson’s  ratio  cb,  can  be  defined  in  card  4,  col.    8,
default = PRBA
TAU1 
*MAT_LAMINATED_COMPOSITE_FABRIC 
DESCRIPTION
𝜏1,  stress  limit  of  the  first  slightly  nonlinear  part  of  the  shear 
stress versus shear strain curve.  The values 𝜏1 and 𝛾1 are used to 
define  a  curve  of  shear  stress  versus  shear  strain.    These  values
are input if FS, defined below, is set to a value of -1. 
GAMMA1 
𝛾1,  strain  limit  of  the  first  slightly  nonlinear  part  of  the  shear
stress versus engineering shear strain curve. 
GAB 
GT.0.0:  𝐺𝑎𝑏, shear modulus ab direction 
LT.0.0:  Load curve ID or Table ID = (-GAB) 
Load Curve. When (-GAB) is equal to a Load curve ID, 
it is taken as defining the elastic shear stress vs.  shear
strain behavior in ab direction. 
Tabular Data. When (-GAB) is equal to a a Table ID, it 
defines for each strain rate value a Load curve ID giv-
ing the elastic shear stress vs.  shear strain behavior in
ab direction. 
Logarithmically  Defined  Tables.  If  the  first  elastic 
shear  stress  vs.    shear  strain  curve  in  the  table  corre-
sponds  to  a  negative  strain  rate,  LS-DYNA  assumes 
that  the  natural  logarithm  of  the  strain  rate  value  is
used for all shear stress-shear strain curves. 
GBC 
GCA 
SLIMT1 
SLIMC1 
SLIMT2 
SLIMC2 
SLIMS 
𝐺𝑏𝑐, shear modulus 𝑏𝑐 
𝐺𝑐𝑎, shear modulus 𝑐𝑎 
Factor  to  determine  the  minimum  stress  limit  after  stress
maximum (fiber tension). 
Factor  to  determine  the  minimum  stress  limit  after  stress
maximum (fiber compression). 
Factor  to  determine  the  minimum  stress  limit  after  stress
maximum (matrix tension). 
Factor  to  determine  the  minimum  stress  limit  after  stress
maximum (matrix compression). 
Factor  to  determine  the  minimum  stress  limit  after  stress
maximum (shear). 
AOPT 
Material axes option (see MAT_OPTION TROPIC_ELASTIC for a
VARIABLE   
DESCRIPTION
more complete description): 
EQ.0.0:  locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES,  and  then  rotated  about  the  shell  ele-
ment normal by an angle BETA. 
EQ.2.0:  globally  orthotropic  with  material  axes  determined  by 
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0:  locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle (BETA) from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  𝐯  with  the 
element normal. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID 
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR). 
TSIZE 
Time step for automatic element deletion. 
ERODS 
Maximum  effective  strain  for  element  layer  failure.    A  value  of 
unity would equal 100% strain. 
GT.0.0: fails when effective strain calculated assuming material
is volume preserving exceeds ERODS (old way). 
LT.0.0:  fails  when  effective  strain  calculated  from  the  full
strain tensor exceeds |ERODS|. 
SOFT 
Softening reduction factor for strength in the crashfront.
transverse shear stiffness
GBC, 
GCA 
D = 0 
D = TSMD 
EPSF 
EPSR
transverse shear strain 
Figure M58-1.  Linear Damage for transverse shear behavior 
  VARIABLE   
DESCRIPTION
FS 
Failure surface type: 
EQ.1.0:  smooth  failure  surface  with  a  quadratic  criterion  for
both  the  fiber  (a)  and  transverse  (b)  directions.    This
option  can  be  used  with  complete  laminates  and  fab-
rics. 
EQ.0.0:  smooth  failure  surface  in  the  transverse  (b)  direction
with  a  limiting  value  in  the  fiber  (a)  direction.    This 
model  is  appropriate  for  unidirectional  (UD)  layered
composites only. 
EQ.-1.:  faceted  failure  surface.    When  the  strength  values  are
reached then damage evolves in tension and compres-
sion for both the fiber and transverse direction.  Shear 
behavior  is  also  considered.    This  option  can  be  used
with complete laminates and fabrics. 
EPSF 
EPSR 
Damage initiation transverse shear strain. 
Final rupture transverse shear strain. 
TSMD 
Transverse shear maximum damage, default = 0.90. 
XP, YP, ZP 
Define coordinates of point 𝐩 for AOPT = 1. 
A1, A2, A3 
Define components of vector 𝐚 for AOPT = 2. 
V1, V2 V3 
Define components of vector 𝐯 for AOPT = 3. 
D1, D2, D3 
Define components of vector 𝐝 for AOPT = 2.
VARIABLE   
BETA 
E11C 
E11T 
E22C 
E22T 
GMS 
XC 
XT 
YC 
YT 
SC 
LCXC 
LCXT 
LCYC 
LCYT 
DESCRIPTION
Material  angle  in  degrees  for  AOPT = 0  and  AOPT = 3.    BETA 
may  be  overridden  on  the  element  card,  see  *ELEMENT_-
SHELL_BETA. 
Strain at longitudinal compressive strength, 𝑎-axis (positive). 
Strain at longitudinal tensile strength, 𝑎-axis. 
Strain at transverse compressive strength, 𝑏-axis. 
Strain at transverse tensile strength, 𝑏-axis. 
Engineering shear strain at shear strength, 𝑎𝑏 plane. 
Longitudinal compressive strength (positive value). 
Longitudinal tensile strength, see below. 
Transverse  compressive  strength,  𝑏-axis  (positive  value),  see 
below. 
Transverse tensile strength, 𝑏-axis, see below. 
Shear strength, 𝑎𝑏 plane, see below. 
Load curve ID defining longitudinal compressive strength XC vs.
strain rate (XC is ignored with that option).  If the first strain rate
value  in  the  curve  is  negative,  it  is  assumed  that  all  strain  rate
values are given as natural logarithm of the strain rate. 
Load curve ID defining longitudinal tensile strength XT vs.  strain
rate (XT is ignored with that option) If the first strain rate value in
the curve is negative, it is assumed that all  strain rate values are
given as natural logarithm of the strain rate. 
Load  curve  ID  defining  transverse  compressive  strength  YC  vs.
strain rate (YC is ignored with that option) If the first strain rate
value  in  the  curve  is  negative,  it  is  assumed  that  all  strain  rate
values are given as natural logarithm of the strain rate. 
Load  curve  ID  defining  transverse  tensile  strength  YT  vs.    strain
rate (YT is ignored with that option) If the first strain rate value in
the curve is negative, it is assumed that all  strain rate values are
given as natural logarithm of the strain rate.
LCSC 
LCTAU 
LCGAM 
*MAT_LAMINATED_COMPOSITE_FABRIC 
DESCRIPTION
Load  curve  ID  defining  shear  strength  SC  vs.    strain  rate  (SC  is
ignored with that option) If the first strain rate value in the curve
is  negative,  it  is  assumed  that  all  strain  rate  values  are  given  as
natural logarithm of the strain rate. 
Load  curve  ID  defining  TAU1  vs.    strain  rate  (TAU1  is  ignored
with that option).  This value is only used for FS = -1. 
If the first strain rate value in the curve is negative, it is assumed
that  all  strain  rate  values  are  given  as  natural  logarithm  of  the 
strain rate. 
Load  curve  ID  defining  GAMMA1  vs.    strain  rate  (GAMMA1  is
ignored with that option).  This value is only used for FS = -1. 
If the first strain rate value in the curve is negative, it is assumed
that  all  strain  rate  values  are  given  as  natural  logarithm  of  the
strain rate. 
DT 
Strain rate averaging option. 
EQ.0.0: Strain rate is evaluated using a running average. 
LT.0.0:  Strain  rate  is  evaluated  using  average  of  last  11  time
steps.  
GT.0.0:  Strain rate is averaged over the last DT time units. 
Load curve ID defining E11C vs.  strain rate (E11C is ignored with
that option) If the first strain rate value in the curve is negative, it
is  assumed  that  all  strain  rate  values  are  given  as  natural
logarithm of the strain rate. 
Load curve ID defining E11T vs.  strain rate (E11T is ignored with
that option) If the first strain rate value in the curve is negative, it
is  assumed  that  all  strain  rate  values  are  given  as  natural
logarithm of the strain rate. 
Load curve ID defining E22C vs.  strain rate (E22C is ignored with
that option) If the first strain rate value in the curve is negative, it
is  assumed  that  all  strain  rate  values  are  given  as  natural
logarithm of the strain rate. 
Load curve ID defining E22T vs.  strain rate (E22T is ignored with
that option) If the first strain rate value in the curve is negative, it
is  assumed  that  all  strain  rate  values  are  given  as  natural
logarithm of the strain rate. 
LCE11C 
LCE11T 
LCE22C 
LCE22T
DESCRIPTION
Load curve ID defining GMS vs.  strain rate (GMS is ignored with 
that option) If the first strain rate value in the curve is negative, it
is  assumed  that  all  strain  rate  values  are  given  as  natural
logarithm of the strain rate. 
Load curve ID defining ERODS vs.  strain rate (ERODS is ignored 
with  that  option).    The  full  strain  tensor  is  used  to  compute  the
equivalent strain (new option).  If the first strain rate value in the
curve is negative, it is assumed that all strain rate values are given
as natural logarithm of the strain rate. 
  VARIABLE   
LCGMS 
LCEFS 
Remarks: 
Parameters  to  control  failure  of  an  element  layer  are:  ERODS,  the  maximum  effective 
strain,  i.e.,  maximum  1 = 100%  straining.    The  layer  in  the  element  is  completely 
removed  after  the  maximum  effective  strain  (compression/tension  including  shear)  is 
reached. 
The stress limits are factors used to limit the stress in the softening part to a given value, 
𝜎min = SLIM𝑥𝑥 × strength, 
thus,  the  damage  value  is  slightly  modified  such  that    elastoplastic  like  behavior  is 
achieved with the threshold stress.  The SLIMxx fields may range between 0.0 and 1.0.  
With  a  factor  of  1.0,  the  stress  remains  at  a  maximum  value  identical  to  the  strength, 
which  is  similar  to  ideal  elastoplastic  behavior.    For  tensile  failure  a  small  value  for 
SLIMTx is often reasonable; however, for compression SLIMCx = 1.0 is preferred.  This 
is also valid for the corresponding shear value. 
If SLIMxx is smaller than 1.0, then localization can be observed depending on the total 
behavior  of  the  lay-up.    If  the  user  is  intentionally  using  SLIMxx < 1.0,  it  is  generally 
recommended to avoid a drop to zero and set the value to something in between 0.05 
and 0.10.  Then elastoplastic behavior is achieved in the limit which often leads to less 
numerical problems.  Defaults for SLIM𝑥𝑥 = 10−8. 
The crashfront-algorithm is started if and only if a value for TSIZE is input.  Note that 
time step size, with element elimination after the actual time step becomes smaller than 
TSIZE. 
The  damage  parameters  can  be  written  to  the  post  processing  database  for  each 
integration point as the first three additional element variables and can be visualized.
τ 
TAU1 
SC 
GAMMA1 
GMS 
SLIMS = 1.0 
SLIMS = 0.9 
SLIMS = 0.6 
γ 
Figure M58-2.  Stress-strain diagram for shear 
Material models with FS = 1 or FS = -1 are favorable for complete laminates and fabrics, 
as all directions are treated in a similar fashion. 
For material model FS = 1 an interaction between normal stresses and the shear stresses 
is assumed for the evolution of damage in the a and b-directions.  For the shear damage 
is  always  the  maximum  value  of  the  damage  from  the  criterion  in  a  or  b-direction  is 
taken. 
For  material  model  FS = -1  it  is  assumed  that  the  damage  evolution  is  independent  of 
any of the other stresses.  A coupling is only present via the elastic material parameters 
and the complete structure. 
In tensile and compression directions and in a as well as in b- direction different failure 
surfaces  can  be  assumed.    The  damage  values,  however,  increase  only  also  when  the 
loading direction changes. 
Special control of shear behavior of fabrics: 
For fabric materials a nonlinear stress strain curve for the shear part for failure surface 
FS = -1 can be assumed as given below.  This is not possible for other values of FS. 
The curve, shown in Figure M58-2 is defined by three points:
1. 
2. 
3. 
the origin (0,0) is assumed,  
the limit of the first slightly nonlinear part (must be input), stress  (TAU1) and 
strain (GAMMA1), see below. 
the shear strength at failure and shear strain at failure. 
In  addition  a  stress  limiter  can  be  used  to  keep  the  stress  constant  via  the  SLIMS 
parameter.    This  value  must  be  less  or  equal  1.0  but  positive,  and  leads  to  an 
elastoplastic  behavior  for  the  shear  part.    The  default  is  10−8,  assuming  almost  brittle 
failure once the strength limit SC is reached.
*MAT_COMPOSITE_FAILURE_{OPTION}_MODEL 
This is Material Type 59. 
Available options include: 
SHELL 
SOLID  
SPH 
depending on the element type the material is to be used with, see *PART. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
EA 
F 
3 
Variable 
GAB 
GBC 
GCA 
Type 
F 
F 
F 
  Card 3 
Variable 
1 
XP 
Type 
F 
  Card 4 
Variable 
1 
V1 
Type 
F 
2 
YP 
F 
2 
V2 
F 
3 
ZP 
F 
3 
V3 
F 
4 
EB 
F 
4 
KF 
F 
4 
A1 
F 
4 
D1 
F 
5 
EC 
F 
5 
6 
7 
8 
PRBA 
PRCA 
PRCB 
F 
6 
F 
7 
F 
8 
AOPT 
MACF 
F 
I 
5 
A2 
F 
5 
D2 
F 
6 
A3 
F 
6 
D3 
F 
7 
8 
7 
8 
BETA
Card 5 for SHELL Keyword Option. 
  Card 5 
1 
2 
3 
4 
Variable 
TSIZE 
ALP 
SOFT 
FBRT 
Type 
F 
F 
F 
F 
Card 6 for SHELL Keyword Option. 
  Card 6 
Variable 
1 
XC 
Type 
F 
2 
XT 
F 
3 
YC 
F 
4 
YT 
F 
5 
SR 
F 
5 
SC 
F 
7 
8 
6 
SF 
F 
6 
7 
8 
Card 5 for SPH and SOLID Keyword Options. 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SBA 
SCA 
SCB 
XXC 
YYC 
ZZC 
Type 
F 
F 
F 
F 
F 
F 
Card 6 for SPH and SOLID Keyword Options. 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
XXT 
YYT 
ZZT 
Type 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
EA 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Density 
𝐸𝑎, Young’s modulus - longitudinal direction
EB 
EC 
PRBA 
PRCA 
PRCB 
GAB 
GBC 
GCA 
KF 
AOPT 
*MAT_COMPOSITE_FAILURE_{OPTION}_MODEL 
DESCRIPTION
𝐸𝑏, Young’s modulus - transverse direction 
𝐸𝑐, Young’s modulus - normal direction 
𝜈𝑏𝑎, Poisson’s ratio ba 
𝜈𝑐𝑎, Poisson’s ratio ca 
𝜈𝑐𝑏, Poisson’s ratio cb 
𝐺𝑎𝑏, Shear Modulus 
𝐺𝑏𝑐, Shear Modulus 
𝐺𝑐𝑎, Shear Modulus 
Bulk modulus of failed material 
Material  axes  option    (SPH  particles  only  support
AOPT = 2.0): 
EQ.0.0:  locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES, and then, for shells only, rotated about 
the shell element normal by an angle BETA. 
EQ.1.0:  locally orthotropic with material axes determined by a
point  in  space  and  the  global  location  of  the  element
center;  this  is  the  𝑎-direction.    This  option  is  for  solid 
elements only. 
EQ.2.0:  globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0:  locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element 
defined  by  the  cross  product  of  the  vector  𝐯  with  the 
element normal. 
EQ.4.0:  locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector  𝐯,  and 
an originating point, 𝐩, which define the centerline ax-
is.  This option is for solid elements only. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
VARIABLE   
DESCRIPTION
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
MACF 
Material axes change flag for brick elements. 
EQ.1:  No change, default, 
EQ.2:  switch material axes 𝑎 and 𝑏, 
EQ.3:  switch material axes 𝑎 and 𝑐, 
EQ.4:  switch material axes 𝑏 and 𝑐. 
XP YP ZP 
Define coordinates of point 𝐩 for AOPT = 1 and 4. 
A1 A2 A3 
Define components of vector 𝐚 for AOPT = 2. 
V1 V2 V3 
Define components of vector 𝐯 for AOPT = 3 and 4. 
D1 D2 D3 
Define components of vector 𝐝 for AOPT = 2: 
BETA 
Material  angle  in  degrees  for  AOPT = 0  (shells  only)  and 
AOPT = 3,  may  be  overridden  on  the  element  card,  see  *ELE-
MENT_SHELL_BETA or *ELEMENT_SOLID_ORTHO. 
TSIZE 
Time step for automatic element deletion 
ALP 
SOFT 
FBRT 
SR 
SF 
XC 
XT 
YC 
YT 
Nonlinear shear stress parameter 
Softening reduction factor for strength in crush 
Softening of fiber tensile strength 
𝑠𝑟, reduction factor (default = 0.447) 
𝑠𝑓 , softening factor (default = 0.0) 
Longitudinal compressive strength, 𝑎-axis (positive value). 
Longitudinal tensile strength, 𝑎-axis 
Transverse compressive strength, 𝑏-axis (positive value). 
Transverse tensile strength, 𝑏-axis
*MAT_COMPOSITE_FAILURE_{OPTION}_MODEL 
DESCRIPTION
SC 
Shear strength, 𝑎𝑏 plane: 
GT.0.0:  faceted failure surface theory, 
LT.0.0:  ellipsoidal failure surface theory. 
SBA 
SCA 
SCB 
XXC 
YYC 
ZZC 
XXT 
YYT 
ZZT 
In plane shear strength. 
Transverse shear strength. 
Transverse shear strength. 
Longitudinal compressive strength 𝑎-axis (positive value). 
Transverse compressive strength 𝑏-axis (positive value). 
Normal compressive strength 𝑐-axis (positive value). 
Longitudinal tensile strength 𝑎-axis. 
Transverse tensile strength 𝑏-axis. 
Normal tensile strength 𝑐-axis.
*MAT_ELASTIC_WITH_VISCOSITY 
This  is  Material  Type  60  which  was  developed  to  simulate  forming  of  glass  products 
(e.g., car windshields) at high temperatures.  Deformation is by viscous flow but elastic 
deformations  can  also  be  large.    The  material  model,  in  which  the  viscosity  may  vary 
with temperature, is suitable for treating a wide range of viscous flow problems and is 
implemented for brick and shell elements. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
V0 
F 
3 
4 
A 
F 
4 
5 
B 
F 
5 
6 
C 
F 
6 
7 
8 
LCID 
F 
7 
8 
Variable 
PR1 
PR2 
PR3 
PR4 
PR5 
PR6 
PR7 
PR8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
  Card 3 
Variable 
1 
T1 
Type 
F 
  Card 4 
Variable 
1 
V1 
Type 
F 
2 
T2 
F 
2 
V2 
F 
3 
T3 
F 
3 
V3 
F 
4 
T4 
F 
4 
V4 
F 
5 
T5 
F 
5 
V5 
F 
6 
T6 
F 
6 
V6 
F 
7 
T7 
F 
7 
V7 
F 
8 
T8 
F 
8 
V8
Variable 
1 
E1 
Type 
F 
  Card 6 
1 
*MAT_ELASTIC_WITH_VISCOSITY 
2 
E2 
F 
2 
3 
E3 
F 
3 
4 
E4 
F 
4 
5 
E5 
F 
5 
6 
E6 
F 
6 
7 
E7 
F 
7 
8 
E8 
F 
8 
Variable 
ALPHA1 
ALPHA2 
ALPHA3 
ALPHA4 
ALPHA5 
ALPHA6 
ALPHA7 
ALPHA8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
V0 
A 
B 
C 
LCID 
T1, T2, 
…, TN 
PR1, PR2, 
…, PRN 
V1, V2, 
…, VN 
2-346 (EOS) 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Temperature  independent  dynamic  viscosity  coefficient,  V0.    If 
defined,  the  temperature  dependent  viscosity  defined  below  is
skipped, see type (i) and (ii) definitions for viscosity below. 
Dynamic  viscosity  coefficient,  see  type  (i)  and  (ii)  definitions
below. 
Dynamic  viscosity  coefficient,  see  type  (i)  and  (ii)  definitions
below. 
Dynamic  viscosity  coefficient,  see  type  (i)  and  (ii)  definitions
below. 
Load  curve    defining  viscosity  versus 
temperature, see type (iii).  (Optional) 
Temperatures, define up to 8 values 
Poisson’s ratios for the temperatures Ti 
Corresponding  dynamic  viscosity  coefficients  (define  only  one  if
VARIABLE   
DESCRIPTION
E1, E2, 
…, EN 
Corresponding  Young’s  moduli  coefficients  (define  only  one  if 
not varying with temperature) 
Corresponding thermal expansion coefficients 
ALPHA1, …, 
ALPHAN. 
Remarks: 
Volumetric behavior is treated as linear elastic.  The deviatoric strain rate is considered 
to be the sum of elastic and viscous strain rates: 
′ = 𝛆̇elastic
𝛆̇total
′
′
+ 𝛆̇viscous
=
𝛔̇′
2𝐺
+  
𝛔′
2𝜈
where G is the elastic shear modulus, v is the viscosity coefficient, and bold indicates a 
tensor.  The stress increment over one timestep dt is 
𝑑𝜎 ′  = 2𝐺𝜺̇total𝑑𝑡 −
𝑑𝑡 σ′ 
The  stress  before  the  update  is  used  for  σ′.    For  shell  elements  the  through-thickness 
strain rate is calculated as follows. 
𝑑𝜎33 = 0 = 𝐾(𝜀̇11 + 𝜀̇22 + 𝜀̇33)𝑑𝑡 + 2𝐺𝜀′̇
33𝑑𝑡 −
𝑑𝑡𝜎′33 
where the subscript ij = 33 denotes the through-thickness direction and K is the elastic 
bulk modulus.  This leads to: 
𝐺)
𝑎 =
𝜀̇33 = −𝑎(𝜀̇11 + 𝜀̇22) + 𝑏𝑝 
(𝐾 − 2
(𝐾 + 4
𝐺𝑑𝑡
𝜐(𝐾 + 4
𝑏 =
𝐺)
𝐺)
in which p is the pressure defined as the negative of the hydrostatic stress. 
The variation of viscosity with temperature can be defined in any one of the 3 ways. 
(i) 
Constant,  V = V0    Do  not  define  constants,  A,  B,  and  C  or  the  piecewise 
curve.(leave card 4 blank) 
(ii) 
V = V0 × 10
(A/(T-B) + C)
(iii) 
Piecewise curve: define the variation of viscosity with temperature. 
NOTE:  Viscosity is inactive during dynamic re-
laxation.
*MAT_ELASTIC_WITH_VISCOSITY_CURVE 
This  is  Material  Type  60  which  was  developed  to  simulate  forming  of  glass  products 
(e.g., car windshields) at high temperatures.  Deformation is by viscous flow but elastic 
deformations  can  also  be  large.    The  material  model,  in  which  the  viscosity  may  vary 
with temperature, is suitable for treating a wide range of viscous flow problems and is 
implemented  for  brick  and  shell  elements.    Load  curves  are  used  to  represent  the 
temperature  dependence  of  Poisson’s  ratio,  Young’s  modulus,  the  coefficient  of 
expansion, and the viscosity. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
V0 
F 
3 
4 
A 
F 
4 
5 
B 
F 
5 
6 
C 
F 
6 
7 
8 
LCID 
F 
7 
8 
Variable 
PR_LC 
YM_LC 
A_LC 
V_LC 
V_LOG 
Type 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
V0 
A 
B 
C 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Temperature  independent  dynamic  viscosity  coefficient,  V0.    If 
defined,  the  temperature  dependent  viscosity  defined  below  is
skipped, see type (i) and (ii) definitions for viscosity below. 
Dynamic  viscosity  coefficient,  see  type  (i)  and  (ii)  definitions
below. 
Dynamic  viscosity  coefficient,  see  type  (i)  and  (ii)  definitions
below. 
Dynamic  viscosity  coefficient,  see  type  (i)  and  (ii)  definitions 
below.
VARIABLE   
DESCRIPTION
Load  curve    defining  factor  on  dynamic 
viscosity versus temperature, see type (iii).  (Optional). 
Load  curve    defining  Poisson’s  ratio  as  a 
function of temperature. 
Load curve  defining Young’s modulus as 
a function of temperature. 
Load  curve    defining  the  coefficient  of 
thermal expansion as a function of temperature. 
Load  curve    defining  the  dynamic 
viscosity as a function of temperature. 
Flag for the form of V_LC.  If V_LOG = 1.0, the value specified in 
V_LC  is  the  natural  logarithm  of  the  viscosity,  ln(V).    The  value
interpolated  from  the  curve  is  then  exponentiated  to  obtain  the
viscosity.    If  V_LOG = 0.0,  the  value  is  the  viscosity.    The 
logarithmic form is useful if the value of the viscosity changes by
orders of magnitude over the temperature range of the data. 
LCID 
PR_LC 
YM_LC 
A_LC 
V_LC 
V_LOG 
Remarks: 
Volumetric behavior is treated as linear elastic.  The deviatoric strain rate is considered 
to be the sum of elastic and viscous strain rates: 
′ = ε̇elastic
ε̇total
′
′
+ ε̇viscous
=  
𝝈̇ ′
2𝐺
+  
σ′
2𝜈
where G is the elastic shear modulus, v is the viscosity coefficient, and bold~ indicates a 
tensor.  The stress increment over one timestep dt is 
𝑑𝝈′ = 2𝐺ε̇total
′
 𝑑𝑡 −
 𝑑𝑡 𝝈′ 
The  stress  before  the  update  is  used  for  σ′.    For  shell  elements  the  through-thickness 
strain rate is calculated as follows. 
𝑑𝜎33 = 0 = 𝐾(𝜀̇11 + 𝜀̇22 + 𝜀̇33)𝑑𝑡 + 2𝐺𝜀′̇
33𝑑𝑡 −
𝑑𝑡𝜎′33 
where the subscript ij = 33 denotes the through-thickness direction and K is the elastic 
bulk modulus.  This leads to: 
𝜀̇33 = −𝑎(𝜀̇11 + 𝜀̇22) + 𝑏𝑝
𝑎 =
𝑏 =
𝐺)
𝐺)
(𝐾 − 2
(𝐾 + 4
𝐺𝑑𝑡
𝜐(𝐾 + 4
𝐺)
in which p is the pressure defined as the negative of the hydrostatic stress. 
The variation of viscosity with temperature can be defined in any one of the 3 ways. 
(i) 
(ii) 
(iii) 
Constant,  V = V0  Do  not  define  constants,  A,  B,  and  C  or  the  piecewise 
curve.(leave card 4 blank) 
V = V0 × 10(A/(T-B) + C) 
Piecewise curve: define the variation of viscosity with temperature. 
Note: Viscosity is inactive during dynamic relaxation.
*MAT_KELVIN-MAXWELL_VISCOELASTIC 
This  is  Material  Type  61.    This  material  is  a  classical  Kelvin-Maxwell  model  for 
modeling  viscoelastic  bodies,  e.g.,  foams.    This  model  is  valid  for  solid  elements  only.  
See also notes below. 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
BULK 
Type 
A8 
F 
F 
4 
G0 
F 
5 
GI 
F 
6 
DC 
F 
7 
FO 
F 
8 
SO 
F 
Default 
none 
none 
none 
none 
none 
0.0 
0.0 
0.0 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density 
BULK 
Bulk modulus (elastic) 
G0 
GI 
DC 
FO 
Short-time shear modulus, G0 
Long-time (infinite) shear modulus, G∞ 
Maxwell decay constant, β[FO = 0.0] or 
Kelvin relaxation constant, τ [FO = 1.0] 
Formulation option: 
EQ.0.0:  Maxwell, 
EQ.1.0:  Kelvin.
VARIABLE   
SO 
DESCRIPTION
Strain  (logarithmic)  output  option  to  control  what  is  written  as
component 7 to the d3plot database.  (LS-PrePost always blindly 
labels  this  component  as  effective  plastic  strain.)    The  maximum
values are updated for each element each time step: 
EQ.0.0:  maximum  principal  strain  that  occurs  during  the
calculation, 
EQ.1.0:  maximum magnitude of the principal strain values that
occurs during the calculation, 
EQ.2.0:  maximum  effective  strain  that  occurs  during  the
calculation. 
Remarks: 
The shear relaxation behavior is described for the Maxwell model by: 
A Jaumann rate formulation is used 
𝐺(𝑡) = 𝐺 + (𝐺0 − 𝐺∞)𝑒−𝛽𝑡 
∇
′ = 2 ∫ 𝐺(𝑡 − 𝜏)  𝐷′𝑖𝑗(𝜏)𝑑𝑡
ij
 𝑡
  0
∇
𝑖𝑗, and the strain rate Dij .  
where the prime denotes the deviatoric part of the stress rate, 𝜎
For the Kelvin model the stress evolution equation is defined as: 
𝑠 ̇𝑖𝑗 +
𝑠𝑖𝑗 = (1 + 𝛿𝑖𝑗)𝐺0𝑒 ̇𝑖𝑗 + (1 + 𝛿𝑖𝑗)
𝐺∞
𝑒 ̇𝑖𝑗 
The strain data as written to the LS-DYNA database may be used to predict damage, see 
[Bandak 1991].
*MAT_VISCOUS_FOAM 
This  is  Material  Type  62.    It  was  written  to  represent  the  Confor  Foam  on  the  ribs  of 
EuroSID  side  impact  dummy.    It  is  only  valid  for  solid  elements,  mainly  under 
compressive loading. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E1 
F 
4 
N1 
F 
5 
V2 
F 
6 
E2 
F 
7 
N2 
F 
8 
PR 
F 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Initial Young’s modulus (E1) 
Exponent in power law for Young’s modulus (n1) 
Viscous coefficient (V2) 
Elastic modulus for viscosity (E2), see notes below. 
Exponent in power law for viscosity (n2) 
Poisson’s ratio, ν 
RO 
E1 
N1 
V2 
E2 
N2 
PR 
Remarks: 
The  model  consists  of  a  nonlinear  elastic  stiffness  in  parallel  with  a  viscous  damper.  
The elastic stiffness is  intended to limit total crush while the viscosity absorbs energy.  
The stiffness E2 exists to prevent timestep problems.  It is used for time step calculations 
𝑡   is  smaller  than  E2.    It  has  to  be  carefully  chosen  to  take  into  account  the 
a  long  as  𝐸1
stiffening effects of the viscosity.  Both E1 and V2 are nonlinear with crush as follows: 
𝑡 = 𝐸1(𝑉−𝑛1) 
𝐸1
𝑡 = 𝑉2|1 − 𝑉|𝑛2 
𝑉2
where viscosity generates a shear stress given by
𝛾̇ is the engineering shear strain rate, and V is the relative volume defined by the ratio 
of the current to initial volume.   
𝜏 = 𝑉2𝛾̇ 
Table showing typical values (units of N, mm, s): 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
E1 
4 
N1 
5 
V2 
6 
E2 
7 
N2 
8 
PR 
Value 
0.0036 
4.0 
0.0015 
100.0 
0.2 
0.05
*MAT_CRUSHABLE_FOAM 
This is Material Type 63 which is dedicated to modeling crushable foam with optional 
damping  and  tension  cutoff.    Unloading  is  fully  elastic.    Tension  is  treated  as  elastic-
perfectly-plastic at the tension cut-off value.  A modified version of this model, *MAT_-
MODIFIED_CRUSHABLE_FOAM includes strain rate effects. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
6 
7 
8 
LCID 
TSC 
DAMP 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
0.0 
0.10 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
LCID 
TSC 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s modulus 
Poisson’s ratio 
Load  curve  ID  defining  yield  stress  versus  volumetric  strain,  𝛾, 
see Figure M63-1. 
Tensile  stress  cutoff.    A  nonzero,  positive  value  is  strongly
recommended for realistic behavior. 
DAMP 
Rate  sensitivity  via  damping  coefficient  (.05 <    recommended 
value < .50).
Stress increases at
higher strain rates
Volumetric Strain
Figure M63-1.  Behavior of strain rate sensitive crushable foam.  Unloading is
elastic  to  the  tension  cutoff.    Subsequent  reloading  follows  the  unloading
curve
Remarks: 
The volumetric strain is defined in terms of the relative volume, V, as: 
𝛾 = 1 − 𝑉 
The relative volume is defined as the ratio of the current to the initial volume.  In place 
of  the  effective  plastic  strain  in  the  d3plot  database,  the  integrated  volumetric  strain 
(natural logarithm of the relative volume) is output.
*MAT_RATE_SENSITIVE_POWERLAW_PLASTICITY 
This  is  Material  Type  64  which  will  model  strain  rate  sensitive  elasto-plastic  material 
with a power law hardening.  Optionally, the coefficients can be defined as functions of 
the effective plastic strain. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
K 
F 
6 
M 
F 
7 
N 
F 
8 
E0 
F 
Default 
none 
none 
none 
none 
none 
0.0001 
none 
0.0002 
  Card 2 
Variable 
1 
VP 
2 
3 
4 
5 
6 
7 
8 
EPS0 
Type 
F 
F 
Default 
0.0 
1.0 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
E 
PR 
K 
M 
Mass density 
Young’s modulus of elasticity 
Poisson’s ratio 
Material  constant,  k.    If  k < 0  the  absolute  value  of  k  is  taken  as 
the  load  curve  number  that  defines  k  as  a  function  of  effective 
plastic strain. 
Strain hardening coefficient, m.  If m < 0 the absolute value of m 
is taken as the load curve number that defines m as a function of
effective plastic strain.
VARIABLE   
DESCRIPTION
N 
E0 
VP 
Strain rate sensitivity coefficient, n.  If n < 0 the absolute value of 
n is taken as the load curve number that defines n as a function of
effective plastic strain. 
Initial strain rate (default = 0.0002) 
Formulation for rate effects: 
EQ.0.0:  Scale yield stress (default) 
EQ.1.0:  Viscoplastic formulation 
EPS0 
Quasi-static threshold strain rate.  See description under *MAT_-
015. 
Remarks: 
This material model follows a constitutive relationship of the form: 
𝜎 = 𝑘𝜀𝑚𝜀̇𝑛 
where 𝜎 is the yield stress,  𝜀 is the effective plastic strain,  𝜀̇ is the effective total strain 
rate (VP = 0), respectively the effective plastic strain rate (VP = 1),  and the constants k, 
m, and n can be expressed as functions of effective plastic strain or can be constant with 
respect to the plastic strain.  The case of no strain hardening can be obtained by setting 
the exponent of the plastic strain equal to a very small positive value, i.e.  0.0001. 
This  model  can  be  combined  with  the  superplastic  forming  input  to  control  the 
magnitude  of  the  pressure  in  the  pressure  boundary  conditions  in  order  to  limit  the 
effective  plastic  strain  rate  so  that  it  does  not  exceed  a  maximum  value  at  any 
integration point within the model. 
A  fully  viscoplastic  formulation  is  optional.    An  additional  cost  is  incurred  but  the 
improvement is results can be dramatic.
*MAT_MODIFIED_ZERILLI_ARMSTRONG 
This  is  Material  Type  65  which  is  a  rate  and  temperature  sensitive  plasticity  model 
which is sometimes preferred in ordnance design calculations. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
  Card 2 
Variable 
1 
C1 
Type 
F 
  Card 3 
Variable 
1 
B1 
Type 
F 
2 
C2 
F 
2 
B2 
F 
3 
G 
F 
3 
C3 
F 
3 
B3 
F 
4 
E0 
F 
4 
C4 
F 
4 
G1 
F 
5 
N 
F 
5 
C5 
F 
5 
G2 
F 
6 
7 
8 
TROOM 
PC 
SPALL 
F 
6 
C6 
F 
6 
G3 
F 
F 
8 
VP 
F 
8 
BULK 
F 
7 
EFAIL 
F 
7 
G4 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
G 
E0 
N 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Shear modulus 
𝜀̇0, factor to normalize strain rate 
n, exponent for bcc metal
TROOM 
Tr, room temperature 
PC 
pc, Pressure cutoff
VARIABLE   
DESCRIPTION
SPALL 
Spall Type: 
EQ.1.0:  minimum pressure limit, 
EQ.2.0:  maximum principal stress, 
EQ.3.0:  minimum pressure cutoff. 
C1, coefficients for flow stress, see notes below. 
C2, coefficients for flow stress, see notes below. 
C3, coefficients for flow stress, see notes below. 
C4, coefficients for flow stress, see notes below. 
C5, coefficients for flow stress, see notes below. 
C6, coefficients for flow stress, see notes below. 
C1 
C2 
C3 
C4 
C5 
C6 
EFAIL 
Failure strain for erosion 
VP 
Formulation for rate effects: 
EQ.0.0:  Scale yield stress (default) 
EQ.1.0:  Viscoplastic formulation 
B1 
B2 
B3 
G1 
G2 
G3 
G4 
B1,  coefficients 
dependency of flow stress yield. 
for  polynomial 
to  represent 
temperature
B2 
B3 
G1,  coefficients  for  defining  heat  capacity  and  temperature
dependency of heat capacity. 
G2 
G3 
G4 
BULK 
Bulk  modulus  defined  for  shell  elements  only.    Do  not  input  for
solid elements.
*MAT_MODIFIED_ZERILLI_ARMSTRONG 
The Armstrong-Zerilli Material Model expresses the flow stress as follows. 
For fcc metals (n = 0), 
𝜎 = 𝐶1 + {𝐶2(𝜀𝑝)
2⁄ [𝑒[−𝐶3+𝐶4ln(𝜀̇∗)]𝑇] + 𝐶5} [
𝜇(𝑇)
𝜇(293)
] 
where, 
𝜀𝑝 = effective plastic strain 
𝜀̇∗ = effective plastic strain rate 
=
𝜀̇
𝜀̇0
and  𝜀̇0 = 1,  1e-3,  1e-6  for  time  units  of  seconds,  milliseconds,  and  microseconds, 
respectively. 
For bcc metals  (n > 0), 
𝜎 = 𝐶1 + 𝐶2𝑒[−𝐶3+𝐶4ln(𝜀̇∗)]𝑇 + [𝐶5(𝜀𝑝)𝑛 + 𝐶6] [
𝜇(𝑇)
𝜇(293)
] 
where 
𝜇(𝑇)
𝜇(293)
= 𝐵1 + 𝐵2𝑇 + 𝐵3𝑇2. 
The  relationship  between  heat  capacity  (specific  heat)  and  temperature  may  be 
characterized by a cubic polynomial equation as follows: 
𝐶𝑝 = 𝐺1 + 𝐺2𝑇 + 𝐺3𝑇2 + 𝐺4𝑇3 
A  fully  viscoplastic  formulation  is  optional.    An  additional  cost  is  incurred  but  the 
improvement is results can be dramatic.
*MAT_LINEAR_ELASTIC_DISCRETE_BEAM 
This is Material Type 66.  This material model is defined for simulating the effects of a 
linear elastic beam by using six springs each acting about one of the six local degrees-of-
freedom.  The two nodes defining a beam may be coincident to give a zero length beam, 
or  offset  to  give  a  finite  length  beam.        For  finite  length  discrete  beams  the  absolute 
value of the variable SCOOR in the SECTION_BEAM input should be set to a value of 
2.0, which causes the local r-axis to be aligned along the two nodes of the beam to give 
physically  correct  behavior.    The  distance  between  the  nodes  of  a  beam  should  not 
affect the behavior of this model.  A triad is used to orient the beam for the directional 
springs.  Translational/rotational stiffness and viscous damping effects are considered 
for a local cartesian system, see notes below.  Applications for this element include the 
modeling of joint stiffnesses. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
4 
5 
6 
7 
8 
TKR 
TKS 
TKT 
RKR 
RKS 
RKT 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
TDR 
TDS 
TDT 
RDR 
RDS 
RDT 
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
7 
8 
Variable 
FOR 
FOS 
FOT 
MOR 
MOS 
MOT 
Type 
F 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass  density,  see  also  “volume”  in  the  *SECTION_BEAM 
definition.
*MAT_LINEAR_ELASTIC_DISCRETE_BEAM 
DESCRIPTION
TKR 
TKS 
TKT 
RKR 
RKS 
RKT 
TDR 
TDS 
TDT 
RDR 
RDS 
RDT 
FOR 
FOS 
FOT 
MOR 
MOS 
MOT 
Translational stiffness along local r-axis, see notes below. 
Translational stiffness along local s-axis. 
Translational stiffness along local t-axis. 
Rotational stiffness about the local r-axis. 
Rotational stiffness about the local s-axis. 
Rotational stiffness about the local t-axis. 
Translational viscous damper along local r-axis.  (Optional) 
Translational viscous damper along local s-axis.  (Optional) 
Translational viscous damper along local t-axis.  (Optional) 
Rotational viscous damper about the local r-axis.  (Optional) 
Rotational viscous damper about the local s-axis.  (Optional) 
Rotational viscous damper about the local t-axis.  (Optional) 
Preload force in r-direction.  (Optional) 
Preload force in s-direction.  (Optional) 
Preload force in t-direction.  (Optional) 
Preload moment about r-axis.  (Optional) 
Preload moment about s-axis.  (Optional) 
Preload moment about t-axis.  (Optional) 
Remarks: 
The formulation of the discrete beam (type  6) assumes that the beam is of zero length 
and  requires  no  orientation  node.    A  small  distance  between  the  nodes  joined  by  the 
beam is permitted.  The local coordinate system which determines (r,s,t) is given by the 
coordinate ID, see *DEFINE_COORDINATE_OPTION, in the cross sectional input, see 
*SECTION_BEAM, where the global system is the default.  The local coordinate system 
axes can rotate with either node of the beam or an average rotation of both nodes .
For null stiffness coefficients, no forces corresponding to these null values will develop.  
The viscous damping coefficients are optional.
*MAT_NONLINEAR_ELASTIC_DISCRETE_BEAM 
This  is  Material  Type  67.    This  material  model  is  defined  for  simulating  the  effects  of 
nonlinear  elastic  and  nonlinear  viscous  beams  by  using  six  springs  each  acting  about 
one  of  the  six  local  degrees-of-freedom.    The  two  nodes  defining  a  beam  may  be 
coincident to give a zero length beam, or offset to give a finite length beam.  For finite 
length  discrete  beams  the  absolute  value  of  the  variable  SCOOR  in  the  SECTION_-
BEAM input should be set to a value of 2.0, which causes the local r-axis to be aligned 
along  the  two  nodes  of  the  beam  to  give  physically  correct  behavior.    The  distance 
between the nodes of a beam should not affect the behavior of this material model.  A 
triad is used to orient the beam for the directional springs.  Arbitrary curves to model 
transitional/ rotational stiffness and damping effects are allowed.  See notes below. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
RO 
LCIDTR 
LCIDTS 
LCIDTT 
LCIDRR 
LCIDRS 
LCIDRT 
Type 
A8 
  Card 2 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
LCIDTDR  LCIDTDS  LCIDTDT  LCIDRDR  LCIDRDS  LCIDRDT 
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
7 
8 
Variable 
FOR 
FOS 
FOT 
MOR 
MOS 
MOT 
Type 
F 
F 
F 
F 
F
Optional Failure Cards.  Cards 4 and 5 must be defined to consider failure; otherwise, 
they are optional. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FFAILR 
FFAILS 
FFAILT  MFAILR  MFAILS  MFAILT 
Type 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
UFAILR 
UFAILS 
UFAILT 
TFAILR 
TFAILS 
TFAILT 
Type 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density, see also volume in *SECTION_BEAM definition. 
LCIDTR 
LCIDTS 
LCIDTT 
LCIDRR 
LCIDRS 
Load curve ID defining translational force resultant along local r-
axis  versus  relative  translational  displacement,  see  Remarks  and
Figure M67-1. 
Load curve ID defining translational force resultant along local s-
axis versus relative translational displacement. 
Load curve ID defining translational force resultant along local t-
axis versus relative translational displacement. 
Load curve ID defining rotational moment resultant about local r-
axis versus relative rotational displacement. 
Load curve ID defining rotational moment resultant about local s-
axis versus relative rotational displacement.
LCIDRT 
LCIDTDR 
LCIDTDS 
LCIDTDT 
LCIDRDR 
LCIDRDS 
LCIDRDT 
FOR 
FOS 
FOT 
MOR 
MOS 
MOT 
FFAILR 
FFAILS 
FFAILT 
MFAILR 
*MAT_NONLINEAR_ELASTIC_DISCRETE_BEAM 
DESCRIPTION
Load curve ID defining rotational moment resultant about local t-
axis versus relative rotational displacement. 
Load  curve  ID  defining  translational  damping  force  resultant
along local r-axis versus relative translational velocity. 
Load  curve  ID  defining  translational  damping  force  resultant
along local s-axis versus relative translational velocity. 
Load  curve  ID  defining  translational  damping  force  resultant
along local t-axis versus relative translational velocity. 
Load  curve  ID  defining  rotational  damping  moment  resultant
about local r-axis versus relative rotational velocity. 
Load  curve  ID  defining  rotational  damping  moment  resultant
about local s-axis versus relative rotational velocity. 
Load  curve  ID  defining  rotational  damping  moment  resultant
about local t-axis versus relative rotational velocity. 
Preload force in r-direction.  (Optional) 
Preload force in s-direction.  (Optional) 
Preload force in t-direction.  (Optional) 
Preload moment about r-axis.  (Optional) 
Preload moment about s-axis.  (Optional) 
Preload moment about t-axis.  (Optional) 
Optional failure parameter.  If zero, the corresponding force, Fr, is 
not considered in the failure calculation. 
Optional failure parameter.  If zero, the corresponding force, Fs, is 
not considered in the failure calculation. 
Optional failure parameter.  If zero, the corresponding force, Ft, is 
not considered in the failure calculation. 
Optional  failure  parameter.    If  zero,  the  corresponding  moment,
Mr, is not considered in the failure calculation.
DESCRIPTION
Optional  failure  parameter.    If  zero,  the  corresponding  moment,
Ms, is not considered in the failure calculation. 
Optional  failure  parameter.    If  zero,  the  corresponding  moment,
Mt, is not considered in the failure calculation. 
Optional 
displacement, ur, is not considered in the failure calculation. 
failure  parameter. 
If  zero, 
the  corresponding
Optional 
displacement, us, is not considered in the failure calculation. 
failure  parameter. 
If  zero, 
the  corresponding
Optional 
displacement, ut, is not considered in the failure calculation. 
failure  parameter. 
If  zero, 
the  corresponding
Optional  failure  parameter.    If  zero,  the  corresponding  rotation,
θr, is not considered in the failure calculation. 
Optional  failure  parameter.    If  zero,  the  corresponding  rotation,
θs, is not considered in the failure calculation. 
Optional  failure  parameter.    If  zero,  the  corresponding  rotation,
θt, is not considered in the failure calculation. 
  VARIABLE   
MFAILS 
MFAILT 
UFAILR 
UFAILS 
UFAILT 
TFAILR 
TFAILS 
TFAILT 
Remarks: 
For null load curve ID’s, no forces are computed. 
The formulation of the discrete beam (type  6) assumes that the beam is of zero length 
and  requires  no  orientation  node.    A  small  distance  between  the  nodes  joined  by  the 
beam is permitted.  The local coordinate system which determines (r,s,t) is given by the 
coordinate ID, see *DEFINE_COORDINATE_OPTION, in the cross sectional input, see 
*SECTION_BEAM, where the global system is the default.  The local coordinate system 
axes can rotate with either node of the beam or an average rotation of both nodes . 
If different behavior in tension and compression is desired in the calculation of the force 
resultants, the load curve(s) must be defined in the negative quadrant starting with the 
most negative displacement then increasing monotonically to the most positive.  If the 
load  curve  behaves  similarly  in  tension  and  compression,  define  only  the  positive 
quadrant.      Whenever  displacement  values  fall  outside  of  the  defined  range,  the 
resultant  forces  will  be  extrapolated.    Figure  M67-1  depicts  a  typical  load  curve  for  a 
force  resultant.    Load  curves  used  for  determining  the  damping  forces  and  moment
resultants  always  act  identically  in  tension  and  compression,  since  only  the  positive 
quadrant values are considered, i.e., start the load curve at the origin [0,0]. 
(a.)
DISPLACEMENT
(b.)
Figure  M67-1.    The  resultant  forces  and  moments  are  determined  by  a  table
lookup.    If  the  origin  of  the  load  curve  is  at  [0,0]  as  in  (b.)  and  tension  and 
compression responses are symmetric. 
|
DISPLACEMENT
|
Catastrophic  failure  based  on  force  resultants  occurs  if  the  following  inequality  is 
satisfied. 
(
𝐹𝑟
fail
𝐹𝑟
)
+ (
𝐹𝑠
fail
𝐹𝑠
)
+ (
𝐹𝑡
fail
𝐹𝑡
)
+ (
𝑀𝑟
fail
𝑀𝑟
)
+ (
𝑀𝑠
fail
𝑀𝑠
)
+ (
𝑀𝑡
fail
𝑀𝑡
)
− 1. ≥ 0. 
After  failure  the  discrete  element  is  deleted.    Likewise,  catastrophic  failure  based  on 
displacement resultants occurs if the following inequality is satisfied: 
(
𝑢𝑟
fail
𝑢𝑟
)
+ (
𝑢𝑠
fail
𝑢𝑠
)
+ (
𝑢𝑡
fail
𝑢𝑡
)
+ (
)
𝜃𝑟
fail
𝜃𝑟
+ (
𝜃𝑠
fail
𝜃𝑠
)
+ (
𝜃𝑡
fail
𝜃𝑡
)
− 1. ≥ 0. 
After failure the discrete element is deleted.  If failure is included either one or both of 
the criteria may be used.
*MAT_NONLINEAR_PLASTIC_DISCRETE_BEAM 
This  is  Material  Type  68.    This  material  model  is  defined  for  simulating  the  effects  of 
nonlinear  elastoplastic,  linear  viscous  behavior  of  beams  by  using  six  springs  each 
acting  about  one  of  the  six  local  degrees-of-freedom.    The  two  nodes  defining  a  beam 
may be coincident to give a zero length beam, or offset to give a finite length beam.  For 
finite  length  discrete  beams  the  absolute  value  of  the  variable  SCOOR  in  the  SEC-
TION_BEAM  input  should  be  set  to  a  value  of  2.0,  which  causes  the  local  r-axis  to  be 
aligned  along  the  two  nodes  of  the  beam  to  give  physically  correct  behavior.    The 
distance  between  the  nodes  of  a  beam  should  not  affect  the  behavior  of  this  material 
model.    A  triad  is  used  to  orient  the  beam  for  the  directional  springs.    Translation-
al/rotational  stiffness  and  damping  effects  can  be  considered.    The  plastic  behavior  is 
modeled  using  force/moment  curves  versus  displacements/rotation.    Optionally, 
failure can be specified based on a force/moment criterion and a displacement rotation 
criterion.  See also notes below. 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
4 
5 
6 
7 
8 
TKR 
TKS 
TKT 
RKR 
RKS 
RKT 
Type 
A8 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TDR 
TDS 
TDT 
RDR 
RDS 
RDT 
Type 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none
Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCPDR 
LCPDS 
LCPDT 
LCPMR 
LCPMS 
LCPMT 
Type 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FFAILR 
FFAILS 
FFAILT  MFAILR  MFAILS  MFAILT 
Type 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
UFAILR 
UFAILS 
UFAILT 
TFAILR 
TFAILS 
TFAILT 
Type 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FOR 
FOS 
FOT 
MOR 
MOS 
MOT 
Type 
F 
F 
F 
F 
F 
F 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density, see also volume on *SECTION_BEAM definition.
VARIABLE   
DESCRIPTION
TKR 
TKS 
TKT 
RKR 
RKS 
RKT 
TDR 
TDS 
TDT 
RDR 
RDS 
RDT 
LCPDR 
LCPDS 
LCPDT 
LCPMR 
LCPMS 
Translational stiffness along local r-axis 
Translational stiffness along local s-axis 
Translational stiffness along local t-axis 
Rotational stiffness about the local r-axis 
Rotational stiffness about the local s-axis 
Rotational stiffness about the local t-axis 
Translational viscous damper along local r-axis 
Translational viscous damper along local s-axis 
Translational viscous damper along local t-axis 
Rotational viscous damper about the local r-axis 
Rotational viscous damper about the local s-axis 
Rotational viscous damper about the local t-axis 
Load  curve  ID-yield  force  versus  plastic  displacement  r-axis.    If 
the curve ID is zero, and if TKR is nonzero, then elastic behavior
is obtained for this component. 
Load  curve  ID-yield  force  versus  plastic  displacement  s-axis.    If 
the curve ID is zero, and if TKS is nonzero, then elastic behavior is
obtained for this component. 
Load  curve  ID-yield  force  versus  plastic  displacement  t-axis.    If 
the curve ID is zero, and if TKT is nonzero, then elastic behavior 
is obtained for this component. 
Load curve ID-yield moment versus plastic rotation r-axis.  If the 
curve  ID  is  zero,  and  if  RKR  is  nonzero,  then  elastic  behavior  is
obtained for this component. 
Load curve ID-yield moment versus plastic rotation s-axis.  If the 
curve  ID  is  zero,  and  if  RKS  is  nonzero,  then  elastic  behavior  is
obtained for this component.
LCPMT 
FFAILR 
FFAILS 
FFAILT 
MFAILR 
MFAILS 
MFAILT 
UFAILR 
UFAILS 
UFAILT 
TFAILR 
TFAILS 
TFAILT 
FOR 
FOS 
*MAT_NONLINEAR_PLASTIC_DISCRETE_BEAM 
DESCRIPTION
Load curve ID-yield moment versus plastic rotation t-axis.  If the 
curve  ID  is  zero,  and  if  RKT  is  nonzero,  then  elastic  behavior  is 
obtained for this component. 
Optional failure parameter.  If zero, the corresponding force, Fr, is 
not considered in the failure calculation. 
Optional failure parameter.  If zero, the corresponding force, Fs, is 
not considered in the failure calculation. 
Optional failure parameter.  If zero, the corresponding force, Ft, is 
not considered in the failure calculation. 
Optional  failure  parameter.    If  zero,  the  corresponding  moment,
Mr, is not considered in the failure calculation. 
Optional  failure  parameter.    If  zero,  the  corresponding  moment,
Ms, is not considered in the failure calculation. 
Optional  failure  parameter.    If  zero,  the  corresponding  moment,
Mt, is not considered in the failure calculation. 
Optional 
displacement, ur, is not considered in the failure calculation. 
failure  parameter. 
If  zero, 
the  corresponding
Optional 
displacement, us, is not considered in the failure calculation. 
failure  parameter. 
If  zero, 
the  corresponding
Optional 
displacement, ut, is not considered in the failure calculation. 
failure  parameter. 
If  zero, 
the  corresponding
Optional  failure  parameter.    If  zero,  the  corresponding  rotation,
θr, is not considered in the failure calculation. 
Optional  failure  parameter.    If  zero,  the  corresponding  rotation,
θs, is not considered in the failure calculation. 
Optional  failure  parameter.    If  zero,  the  corresponding  rotation,
θt, is not considered in the failure calculation. 
Preload force in r-direction.  (Optional) 
Preload force in s-direction.  (Optional)
VARIABLE   
DESCRIPTION
Preload force in t-direction.  (Optional) 
Preload moment about r-axis.  (Optional) 
Preload moment about s-axis.  (Optional) 
Preload moment about t-axis.  (Optional) 
FOT 
MOR 
MOS 
MOT 
Remarks: 
For  the  translational  and  rotational  degrees  of  freedom  where  elastic  behavior  is 
desired, set the load curve ID to zero. 
The plastic displacement for the load curves is defined as: 
plastic displacement = total displacement − yield force/elastic stiffness 
The formulation of the discrete beam (type  6) assumes that the beam is of zero length 
and  requires  no  orientation  node.    A  small  distance  between  the  nodes  joined  by  the 
beam is permitted.  The local coordinate system which determines (r,s,t) is given by the 
coordinate ID  in the cross sectional input, see 
*SECTION_BEAM, where the global system is the default.  The local coordinate system 
axes can rotate with either node of the beam or an average rotation of both nodes . 
Catastrophic  failure  based  on  force  resultants  occurs  if  the  following  inequality  is 
satisfied.   
(
𝐹𝑟
fail
𝐹𝑟
)
+ (
𝐹𝑠
fail
𝐹𝑠
)
+ (
𝐹𝑡
fail
𝐹𝑡
)
+ (
𝑀𝑟
fail
𝑀𝑟
)
+ (
𝑀𝑠
fail
𝑀𝑠
)
+ (
𝑀𝑡
fail
𝑀𝑡
)
− 1. ≥ 0. 
After  failure  the  discrete  element  is  deleted.    Likewise,  catastrophic  failure  based  on 
displacement resultants occurs if the following inequality is satisfied: 
(
𝑢𝑟
fail
𝑢𝑟
)
+ (
𝑢𝑠
fail
𝑢𝑠
)
+ (
𝑢𝑡
fail
𝑢𝑡
)
+ (
)
𝜃𝑟
fail
𝜃𝑟
+ (
𝜃𝑠
fail
𝜃𝑠
)
+ (
𝜃𝑡
fail
𝜃𝑡
)
− 1. ≥ 0.
PLASTIC DISPLACEMENT
Figure  M68-1.    The  resultant  forces  and  moments  are  limited  by  the  yield
definition.    The  initial  yield  point  corresponds  to  a  plastic  displacement  of
zero
After failure the discrete element is deleted.  If failure is included either one or both of 
the criteria may be used.
*MAT_SID_DAMPER_DISCRETE_BEAM 
This is Material Type 69.  The side impact dummy uses a damper that is not adequately 
treated  by  the  nonlinear  force  versus  relative  velocity  curves  since  the  force 
characteristics are dependent on the displacement of the piston.  See also notes below. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
Variable 
1 
C3 
2 
RO 
F 
2 
3 
ST 
F 
3 
STF 
RHOF 
Type 
F 
F 
F 
4 
D 
F 
4 
C1 
F 
5 
R 
F 
5 
C2 
F 
6 
H 
F 
6 
7 
K 
F 
7 
LCIDF 
LCIDD 
F 
F 
8 
C 
F 
8 
S0 
F 
Orifrice Cards.  Include on card per orifice.  Read in up to 15 orifice locations.  Input is 
terminated  when  a  “*”  card  is  found.    On  the  first  card  below  the  optional  input 
parameters SF and DF may be specified.  
  Cards 3 
1 
2 
Variable 
ORFLOC  ORFRAD 
Type 
F 
F 
3 
SF 
F 
4 
DC 
F 
5 
6 
7 
8 
  VARIABLE   
MID 
RO 
ST 
D 
R 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density, see also volume on *SECTION_BEAM definition. 
St, piston stroke.  St must equal or exceed the length of the beam 
element, see Figure M69-1 below. 
d, piston diameter 
R, default orifice radius
H 
K 
C 
C3 
STF 
*MAT_SID_DAMPER_DISCRETE_BEAM 
DESCRIPTION
h, orifice controller position 
K, damping constant 
LT.0.0: |K|  is  the  load  curve  number  ID,  see  *DEFINE_-
CURVE, defining the damping coefficient as a function
of the absolute value of the relative velocity. 
C, discharge coefficient 
Coefficient for fluid inertia term 
k, stiffness coefficient if piston bottoms out 
RHOF 
ρ𝑓𝑙𝑢𝑖𝑑, fluid density 
C1 
C2 
LCIDF 
LCIDD 
C1, coefficient for linear velocity term 
C2, coefficient for quadratic velocity term 
Load curve number ID defining force versus piston displacement,
s,  i.e.,  term  𝑓 (𝑠 + 𝑠0).  Compressive  behavior  is  defined  in  the 
positive quadrant of the force displacement curve.  Displacements
falling  outside  of  the  defined  force  displacement  curve  are
extrapolated.    Care  must  be  taken  to  ensure  that  extrapolated
values are reasonable. 
Load  curve  number  ID  defining  damping  coefficient  versus
piston  displacement,  s,  i.e.,  𝑔(𝑠 + 𝑠0).    Displacements  falling 
outside the defined curve are extrapolated.  Care must be taken to
ensure that extrapolated values are reasonable. 
S0 
Initial  displacement  s0,  typically  set  to  zero. 
displacement corresponds to compressive behavior. 
  A  positive 
ORFLOC 
di, orifice location of ith orifice relative to the fixed end. 
ORFRAD 
ri, orifice radius of ith orifice, if zero the default radius is used. 
SF 
DC 
Scale factor on calculated force.  The default is set to 1.0 
c,  linear  viscous  damping  coefficient  used  after  damper  bottoms
out either in tension or compression.
Remarks: 
As  the  damper  moves,  the  fluid  flows  through  the  open  orifices  to  provide  the 
necessary  damping  resistance.    While  moving  as  shown  in  Figure  M69-1  the  piston 
gradually blocks off and effectively closes the orifices.  The number of orifices and the 
size  of  their  opening  control  the  damper  resistance  and  performance.    The  damping 
force is computed from, 
𝐹 = SF ×
{⎧
⎩{⎨
𝐾𝐴𝑝𝑉𝑝
{⎧𝐶1
⎩{⎨
𝐴0
𝑡 + 𝐶2∣𝑉𝑝∣𝜌fluid
𝐴𝑝
𝐶𝐴0
𝑡 )
⎡(
⎢
⎣
− 1
}⎫
⎤
⎥
⎭}⎬
⎦
}⎫
− 𝑓 (𝑠 + 𝑠0) + 𝑉𝑝𝑔(𝑠 + 𝑠0)
⎭}⎬
where K is a user defined constant or a tabulated function of the absolute value of the 
relative velocity, Vp is the piston velocity, C is the discharge coefficient, Ap is the piston 
𝑡  is the total open areas of orifices at time t, ρfluid is the fluid density, C1 is the 
area, 𝐴0
coefficient for the linear term, and C2 is the coefficient for the quadratic term. 
d4
d3
d2
d1
Piston
Vp
ith Piston Orifice
Orifice Opening Controller
Figure M69-1.  Mathematical model for the Side Impact Dummy damper. 
2Ri - h
In the implementation, the orifices are assumed to be circular with partial covering by 
the  orifice  controller.    As  the  piston  closes,  the  closure  of  the  orifice  is  gradual.    This 
gradual  closure  is  properly  taken  into  account  to  insure  a  smooth  response.    If  the 
piston  stroke  is  exceeded,  the  stiffness  value,  k,  limits  further  movement,  i.e.,  if  the 
damper  bottoms  out  in  tension  or  compression  the  damper  forces  are  calculated  by 
replacing the damper by a bottoming out spring and damper, k and c, respectively.  The
piston  stroke  must  exceed  the  initial  length  of  the  beam  element.    The  time  step 
calculation is based in part on the stiffness value of the bottoming out spring.  A typical 
force versus displacement curve at constant relative velocity is shown in Figure M69-2. 
The  factor,  SF,  which  scales  the  force  defaults  to  1.0  and  is  analogous  to  the  adjusting 
ring on the damper. 
Last orifice
closes.
Force increases as orifice
is gradually covered.
DISPLACEMENT
Figure M69-2.  Force versus displacement as orifices are covered at a constant
relative velocity.  Only the linear velocity term is active.
*MAT_HYDRAULIC_GAS_DAMPER_DISCRETE_BEAM 
This is Material Type 70.  This special purpose element represents a combined hydraulic 
and  gas-filled  damper  which  has  a  variable  orifice  coefficient.    A  schematic  of  the 
damper is shown in Figure M70-1.  Dampers of this type are sometimes used on buffers 
at  the  end  of  railroad  tracks  and  as  aircraft  undercarriage  shock  absorbers.    This 
material can be used only as a discrete beam element.  See also notes below. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
  Card 2 
1 
Variable 
LCID 
Type 
F 
2 
FR 
F 
3 
CO 
F 
3 
4 
N 
F 
4 
SCLF 
CLEAR 
F 
F 
5 
P0 
F 
5 
6 
PA 
F 
6 
7 
AP 
F 
7 
8 
KH 
F 
8 
  VARIABLE   
MID 
RO 
CO 
N 
P0 
PA 
AP 
KH 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density, see also volume in *SECTION_BEAM definition. 
Length of gas column, Co 
Adiabatic constant 
Initial gas pressure, P0 
Atmospheric pressure, Pa 
Piston cross sectional area, Ap 
Hydraulic constant, K 
LCID 
Load  curve  ID,  see  *DEFINE_CURVE,  defining  the  orifice  area, 
a0, versus element deflection.
Orifice
  VARIABLE   
FR 
Oil
Profiled Pin
Gas
Figure M70-1.  Schematic of Hydraulic/Gas damper. 
DESCRIPTION
Return  factor  on  orifice  force.    This  acts  as  a  factor  on  the
hydraulic  force  only  and  is  applied  when  unloading.    It  is
intended to represent a valve that opens when the piston unloads 
to relieve hydraulic pressure.  Set it to 1.0 for no such relief. 
SCLF 
Scale factor on force.  (Default = 1.0) 
CLEAR 
Clearance  (if  nonzero,  no  tensile  force  develops  for  positive
displacements  and  negative  forces  develop  only  after  the
clearance is closed. 
Remarks: 
As the damper is compressed two actions contribute to the force which develops.  First, 
the  gas  is  adiabatically  compressed  into  a  smaller  volume.    Secondly,  oil  is  forced 
through  an  orifice.    A profiled  pin  may occupy  some  of  the  cross-sectional  area  of the 
orifice;  thus,  the  orifice  area  available  for  the  oil  varies  with  the  stroke.    The  force  is 
assumed  proportional  to  the  square  of  the  velocity  and  inversely  proportional  to  the 
available area. 
The equation for this element is: 
𝐹 = SCLF × {𝐾ℎ (
𝑎0
)
+ [𝑃0 (
𝐶0
𝐶0 − 𝑆
)
− 𝑃𝑎] 𝐴𝑝} 
where S is the element deflection and V is the relative velocity across the element.
*MAT_071 
This is Material Type 71.  This model permits elastic cables to be realistically modeled; 
thus, no force will develop in compression. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
LCID 
F 
Default 
none 
none 
none 
none 
5 
F0 
F 
0 
6 
7 
8 
TMAXF0 
TRAMP 
IREAD 
F 
0 
F 
0 
I 
0 
Additional card for IREAD > 1.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OUTPUT 
TSTART 
FRACL0  MXEPS 
MXFRC 
Type 
Default 
I 
0 
F 
0 
F 
0 
F 
F 
1.0E+20 1.0E+20
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
LCID 
F0 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density, see also volume in *SECTION_BEAM definition. 
GT.0.0:  Young’s modulus 
LT.0.0:  Stiffness 
Load  curve  ID,  see  *DEFINE_CURVE,  defining  the  stress  versus 
engineering strain.  (Optional). 
Initial tensile force.  If F0 is defined, an offset is not needed for an
initial tensile force. 
TMAXF0 
Time for which pre-tension force will be held
*MAT_CABLE_DISCRETE_BEAM 
DESCRIPTION
TRAMP 
Ramp-up time for pre-tension force 
IREAD 
Set to 1 to read second line of input 
OUTPUT 
Flag = 1  to  output  axial  strain   
TSTART 
Time at which the ramp-up of pre-tension begins 
FRACL0 
Fraction of initial length that should be reached over time period
of TRAMP.  Corresponding tensile force builds up as necessary to
reach cable length = FRACL0 × L0 at time t = TRAMP. 
MXEPS 
Maximum strain at failure 
MXFRC 
Maximum force at failure 
Remarks: 
The force, F, generated by the cable is nonzero if and only if the cable is tension.  The 
force is given by: 
where ΔL is the change in length  
𝐹 = max(𝐹0 + 𝐾Δ𝐿, 0. ) 
Δ𝐿 = current length − (initial length − offset) 
and the stiffness (E > 0.0 only ) is defined as: 
𝐾 =
𝐸 × area
(initial length − offset)
Note that a constant force element can be obtained by setting: 
although the application of such an element is unknown. 
𝐹0 > 0 and 𝐾 = 0 
The area and offset are defined on either the cross section or element cards.  For a slack 
cable  the  offset  should  be  input  as  a  negative  length.    For  an  initial  tensile  force  the 
offset should be positive. 
If a load curve is specified the Young’s modulus will be ignored and the load curve will 
be used instead.  The points on the load curve are defined as engineering stress versus 
engineering  strain,  i.e.,  the  change  in  length  over  the  initial  length.    The  unloading 
behavior follows the loading.
By  default,  cable  pretension  is  applied  only  at  the  start  of  the  analysis.    If  the  cable  is 
attached to flexible structure, deformation of the structure will result in relaxation of the 
cables, which will therefore lose some or all of the intended preload. 
This can be overcome by using TMAXF0.  In this case, it is expected that the structure 
will deform under the loading from the cables and that this deformation will take time 
to  occur  during  the  analysis.    The  unstressed  length  of  the  cable  will  be  continuously 
adjusted until time TMAXF0 such that the force is maintained at the user-defined pre-
tension force – this is analogous to operation of the pre-tensioning screws in real cables.  
After  time  TMAXF0,  the  unstressed  length  is  fixed  and  the  force  in  the  cable  is 
determined in the normal way using the stiffness and change of length. 
Sudden application of the cable forces at time zero may result in an excessively dynamic 
response  during  pre-tensioning.    A  ramp-up  time  TRAMP  may  optionally  be  defined.  
The cable force ramps up from zero at time TSTART to the full pre-tension F0 at time 
TSTART +  TRAMP.    TMAXF0,  if  set  less  than  TSTART +  TRAMP  by  the  user,  will  be 
internally reset to TSTART + TRAMP. 
If  the  model  does  not  use  dynamic  relaxation,  it  is  recommended  that  damping  be 
applied  during  pre-tensioning  so  that  the  structure  reaches  a  steady  state  by  time 
TMAXF0. 
If  the  model  uses  dynamic  relaxation,  TSTART,  TRAMP,  and  TMAXF0  apply  only 
during dynamic relaxation.  The cable preload at the end of dynamic relaxation carries 
over to the start of the subsequent transient analysis.  
The cable mass will be calculated from length × area × density if VOL is set to zero on 
*SECTION_BEAM.  Otherwise, VOL × density will be used. 
If OUTPUT is set to 1, one additional history variable representing axial strain is output 
to  d3plot  for  the  cable  elements.    This  axial  strain  can  be  plotted  by  LS-PrePost  by 
selecting  the  beam  component  labeled  as  “axial  stress”.    Though  the  label  says  “axial 
stress”, it is actually axial strain. 
If  the  stress-strain  load  curve  option,  LCID,  is  combined  with  preload,  two  types  of 
behavior are available: 
1. 
2. 
If the preload is applied using the TMAXF0/TRAMP method, the initial strain 
is calculated from the stress-strain curve to achieve the desired preload. 
If TMAXF0/TRAMP are not used, the preload force is taken as additional to the 
force calculated from the stress/strain curve.  Thus, the total stress in the cable 
will be higher than indicated by the stress/strain curve.
*MAT_CONCRETE_DAMAGE 
This is Material Type 72.  This model has been used to analyze buried steel reinforced 
concrete  structures  subjected  to  impulsive  loadings.    A  newer  version  of  this  model  is 
available as *MAT_CONCRETE_DAMAGE_REL3 
4 
5 
6 
7 
8 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
PR 
F 
Default 
none 
none 
none 
5 
6 
7 
8 
  Card 2 
1 
Variable 
SIGF 
Type 
F 
2 
A0 
F 
3 
A1 
F 
4 
A2 
F 
Default 
0.0 
0.0 
0.0 
0.0 
  Card 3 
1 
2 
3 
4 
5 
Variable 
A0Y 
A1Y 
A2Y 
A1F 
A2F 
Type 
F 
F 
F 
F 
F 
6 
B1 
F 
7 
B2 
F 
8 
B3 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0
Card 4 
1 
Variable 
PER 
Type 
F 
2 
ER 
F 
3 
4 
5 
6 
7 
8 
PRR 
SIGY 
ETAN 
LCP 
LCR 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
none 
0.0 
none 
none 
  Card 5 
Variable 
Type 
1 
λ 
F 
2 
λ2 
F 
3 
λ3 
F 
4 
λ4 
F 
5 
λ5 
F 
6 
λ6 
F 
7 
λ7 
F 
8 
λ8 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 6 
Variable 
1 
λ9 
2 
3 
4 
5 
6 
7 
8 
λ10 
λ11 
λ12 
λ13 
Type 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
  Card 7 
Variable 
1 
η1 
Type 
F 
2 
η2 
F 
3 
η3 
F 
4 
η4 
F 
5 
η5 
F 
6 
η6 
F 
7 
η7 
F 
8 
η8 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none
Variable 
1 
η9 
*MAT_CONCRETE_DAMAGE 
2 
3 
4 
5 
6 
7 
8 
η10 
η11 
η12 
η13 
Type 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
MID 
RO 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Poisson’s ratio. 
SIGF 
Maximum principal stress for failure. 
A0 
A1 
A2 
A0Y 
A1Y 
A2Y 
A1F 
A2F 
B1 
B2 
B3 
PER 
ER 
Cohesion. 
Pressure hardening coefficient. 
Pressure hardening coefficient. 
Cohesion for yield 
Pressure hardening coefficient for yield limit 
Pressure hardening coefficient for yield limit 
Pressure hardening coefficient for failed material. 
Pressure hardening coefficient for failed material. 
Damage scaling factor. 
Damage scaling factor for uniaxial tensile path. 
Damage scaling factor for triaxial tensile path. 
Percent reinforcement. 
Elastic modulus for reinforcement.
VARIABLE   
DESCRIPTION
PRR 
SIGY 
Poisson’s ratio for reinforcement. 
Initial yield stress. 
ETAN 
Tangent modulus/plastic hardening modulus. 
Load  curve  ID  giving  rate  sensitivity  for  principal  material,  see
*DEFINE_CURVE. 
Load curve ID giving rate sensitivity for reinforcement, see *DE-
FINE_CURVE. 
Tabulated damage function 
Tabulated scale factor. 
LCP 
LCR 
λ1 - λ13 
η1 - η13 
Remarks: 
1.  Cohesion for failed material 𝑎0𝑓 = 0. 
2.  B3 must be positive or zero. 
3.  𝜆𝑛 ≤ 𝜆𝑛+1.  The first point must be zero.
*MAT_CONCRETE_DAMAGE_REL3 
This is Material Type 72R3.  The Karagozian & Case (K&C) Concrete Model - Release III 
is  a  three-invariant  model,  uses  three  shear  failure  surfaces,  includes  damage  and 
strain-rate effects, and has origins based on the Pseudo-TENSOR Model (Material Type 
16).    The  most  significant  user  improvement  provided  by  Release  III  is  a  model 
parameter generation capability, based solely on the unconfined compression strength 
of the concrete.  The implementation of Release III significantly changed the user input, 
thus previous input files using Material Type 72, i.e.  prior to LS-DYNA Version 971, are 
not compatible with the present input format. 
An  open  source  reference,  that  precedes  the  parameter  generation  capability,  is 
provided  in  Malvar  et  al.    [1997].    A  workshop  proceedings  reference,  Malvar  et  al.  
[1996],  is  useful,  but  may  be  difficult  to  obtain.    More  recent,  but  limited  distribution 
reference  materials,  e.g.    Malvar  et  al.    [2000],  may  be  obtained  by  contacting 
Karagozian & Case. 
Seven  card  images  are  required  to  define  the  complete  set  of  model  parameters  for  the 
K&C  Concrete  Model.    An  Equation-of-State  is  also  required  for  the  pressure-volume 
strain  response.    Brief  descriptions  of  all  the  input  parameters  are  provided  below, 
however  it  is  expected  that  this  model  will  be  used  primarily  with  the  option  to 
automatically  generate  the  model  parameters  based  on  the  unconfined  compression 
strength  of  the  concrete.    These  generated  material  parameters,  along  with  the 
generated  parameters  for  *EOS_TABULATED_COMPACTION,  are  written  to  the 
d3hsp  file. 
4 
5 
6 
7 
8 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
PR 
F 
Default 
none 
none 
none
Card 2 
Variable 
1 
FT 
Type 
F 
2 
A0 
F 
3 
A1 
F 
4 
A2 
F 
5 
B1 
F 
6 
7 
8 
OMEGA 
A1F 
F 
F 
Default 
none 
0.0 
0.0 
0.0 
0.0 
none 
0.0 
  Card 3 
Variable 
1 
Sλ 
2 
3 
4 
5 
6 
7 
8 
NOUT 
EDROP 
RSIZE 
UCF 
LCRATE 
LOCWID 
NPTS 
Type 
F 
F 
F 
F 
F 
I 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
λ01 
λ02 
λ03 
λ04 
λ05 
λ06 
λ07 
λ08 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 5 
1 
2 
3 
4 
5 
Variable 
λ09 
λ10 
λ11 
λ12 
λ13 
Type 
F 
F 
F 
F 
F 
6 
B3 
F 
7 
8 
A0Y 
A1Y 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
0.0 
0.0
Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
η01 
η02 
η03 
η04 
η05 
η06 
η07 
η08 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 7 
1 
2 
3 
4 
5 
Variable 
η09 
η10 
η11 
η12 
η13 
Type 
F 
F 
F 
F 
F 
6 
B2 
F 
7 
8 
A2F 
A2Y 
F 
F 
Default 
none 
none 
none 
none 
none 
0.0 
0.0 
0.0 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
PR 
FT 
A0 
A1 
A2 
B1 
Mass density. 
Poisson’s ratio, 𝜈. 
Uniaxial tensile strength, 𝑓𝑡. 
Maximum  shear  failure  surface  parameter,  𝑎0  or  −𝑓𝑐
parameter generation (recommended). 
′  for 
Maximum shear failure surface parameter, 𝑎1. 
Maximum shear failure surface parameter, 𝑎2. 
Compressive damage scaling parameter, 𝑏1 
OMEGA 
Fractional dilatancy, 𝜔. 
A1F 
Sλ 
2-392 (EOS) 
Residual failure surface coefficient, 𝑎1𝑓 .
VARIABLE   
DESCRIPTION
NOUT 
Output selector for effective plastic strain . 
EDROP 
RSIZE 
UCF 
LCRATE 
LOCWID 
NPTS 
λ01 
λ02 
λ03 
λ04 
λ05 
λ06 
λ07 
λ08 
λ09 
λ10 
λ11 
λ12 
Post peak dilatancy decay, 𝑁𝛼. 
Unit conversion factor for length (inches/user-unit), e.g.  39.37 if 
user length unit in meters. 
Unit conversion factor for stress (psi/user-unit), e.g.  145 if  𝑓′𝑐 in 
MPa. 
Define (load) curve number for strain-rate effects; effective strain 
rate  on  abscissa  (negative = tension)  and  strength  enhancement 
on  ordinate.    If  LCRATE  is  set  to  -1,  strain  rate  effects  are
automatically  included,  based  on  equations  provided  in  Wu, 
Crawford, Lan, and Magallanes [2014]. 
Three  times  the  maximum  aggregate  diameter  (input  in  user
length units). 
Number  of  points  in  𝜆  versus  𝜂  damage  relation;  must  be  13 
points. 
1st  value  of  damage  function,  (a.k.a.,  1st  value  of  “modified” 
effective plastic strain; see references for details). 
2nd value of damage function, 
3rd value of damage function, 
4th value of damage function, 
5th value of damage function, 
6th value of damage function, 
7th value of damage function, 
8th value of damage function, 
9th value of damage function, 
10th value of damage function, 
11th value of damage function, 
12th value of damage function,
VARIABLE   
DESCRIPTION
λ13 
B3 
A0Y 
A1Y 
η01 
η02 
η03 
η04 
η05 
η06 
η07 
η08 
η09 
η10 
η11 
η12 
η13 
B2 
A2F 
A2Y 
13th value of damage function. 
Damage scaling coefficient for triaxial tension, 𝑏3. 
Initial yield surface cohesion, 𝑎0𝑦. 
Initial yield surface coefficient, 𝑎1𝑦. 
1st value of scale factor, 
2nd value of scale factor, 
3rd value of scale factor, 
4th value of scale factor, 
5th value of scale factor, 
6th value of scale factor, 
7th value of scale factor, 
8th value of scale factor, 
9th value of scale factor, 
10th value of scale factor, 
11th value of scale factor, 
12th value of scale factor, 
13th value of scale factor. 
Tensile damage scaling exponent, 𝑏2. 
Residual failure surface coefficient, 𝑎2𝑓 . 
Initial yield surface coefficient, 𝑎2𝑦. 
λ, sometimes referred to as “modified” effective plastic strain, is computed internally as 
a function of effective plastic strain, strain rate enhancement factor, and pressure.  η is a 
function of λ as specified by the η vs. λ curve.  The η value, which is always between 0 
and 1, is used to interpolate between the yield failure surface and the maximum failure 
surface,  or  between  the  maximum  failure  surface  and  the  residual  failure  surface, 
depending on whether λ is to the left or right of the first peak in the the η vs. λ curve.   
The  “scaled  damage  measure”  ranges  from  0  to  1  as  the  material  transitions  from  the
yield failure surface to the maximum failure surface, and thereafter ranges from 1 to 2 
as the material ranges from the maximum failure surface to the residual failure surface.  
See the references for details. 
Output of Selected Variables: 
The quantity labeled as “plastic strain” by LS-PrePost is actually the quantity described 
in Table M72-1, in accordance with the  input value of NOUT . 
NOUT 
Function 
Description 
1 
2 
3 
4 
Current shear failure surface radius 
𝛿 = 2𝜆/(𝜆 + 𝜆𝑚) 
𝜎̇𝑖𝑗𝜀̇𝑖𝑗 
𝑝  
𝜎̇𝑖𝑗𝜀̇𝑖𝑗
Scaled damage measure 
Strain energy (rate) 
Plastic strain energy (rate) 
Table M72-1.  Description of quantity labeled “plastic strain” by LS-PrePost. 
An additional six extra history variables as shown in Table M72-2  may be be written by 
setting NEIPH = 6 on the keyword *DATABASE_EXTENT_BINARY.  The extra history 
variables are  labeled as "history var#1" through "history var#6" in LS-PrePost.  
Label 
Description 
history var#1 
Internal energy 
history var#2 
Pressure from bulk viscosity 
history var#3 
Volume in previous time step 
history var#4 
history var#5 
history var#6 
Plastic volumetric strain 
Slope of damage evolution (η vs. λ) 
curve  
“Modified” effective plastic strain (λ) 
Table M72-2.  Extra History Variables for *MAT_072R3 
Sample Input for Concrete: 
As  an  example  of  the  K&C  Concrete  Model  material  parameter  generation,  the 
following  sample  input  for  a  45.4  MPa  (6,580  psi)  unconfined  compression  strength 
concrete  is  provided.    The  basic  units  for  the  provided  parameters  are  length  in 
millimeters (mm), time in milliseconds (msec), and mass in grams (g).  This base unit set 
yields units of force in Newtons (N) and pressure in Mega-Pascals (MPa).
Card 1 
1 
Variable 
MID 
2 
RO 
Type 
72 
2.3E-3 
  Card 2 
Variable 
1 
FT 
2 
A0 
Type 
-45.4 
3 
PR 
3 
A1 
4 
5 
6 
7 
8 
4 
A2 
5 
B1 
6 
7 
8 
OMEGA 
A1F 
  Card 3 
Variable 
1 
Sλ 
2 
3 
4 
5 
6 
7 
8 
NOUT 
EDROP 
RSIZE 
UCF 
LCRATE 
LOCWID 
NPTS 
Type 
3.94E-2
145.0 
723.0 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
λ01 
λ02 
λ03 
λ04 
λ05 
λ06 
λ07 
λ08 
Type 
  Card 5 
1 
2 
3 
4 
5 
Variable 
λ09 
λ10 
λ11 
λ12 
λ13 
6 
B3 
7 
8 
A0Y 
A1Y 
Type
Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
η01 
η02 
η03 
η04 
η05 
η06 
η07 
η08 
Type 
  Card 7 
1 
2 
3 
4 
5 
Variable 
η09 
η10 
η11 
η12 
η13 
6 
B2 
7 
8 
A2F 
A2Y 
Type 
Shear strength enhancement factor versus effective strain rate is given by a curve (*DE-
FINE_CURVE) with LCID 723.  The sample input values, see Malvar & Ross [1998], are 
given in Table M72-3.
Strain-Rate (1/ms) 
Enhancement 
-3.0E+01 
-3.0E-01 
-1.0E-01 
-3.0E-02 
-1.0E-02 
-3.0E-03 
-1.0E-03 
-1.0E-04 
-1.0E-05 
-1.0E-06 
-1.0E-07 
-1.0E-08 
0.0E+00 
3.0E-08 
1.0E-07 
1.0E-06 
1.0E-05 
1.0E-04 
1.0E-03 
3.0E-03 
1.0E-02 
3.0E-02 
1.0E-01 
3.0E-01 
3.0E+01 
9.70 
9.70 
6.72 
4.50 
3.12 
2.09 
1.45 
1.36 
1.28 
1.20 
1.13 
1.06 
1.00 
1.00 
1.03 
1.08 
1.14 
1.20 
1.26 
1.29 
1.33 
1.36 
2.04 
2.94 
2.94 
Table  M72-3.    Enhancement  versus  effective  strain  rate  for  45.4  MPa 
concrete (sample).  When defining curve LCRATE, input negative (tensile) 
values  of  effective  strain  rate  first.    The  enhancement  should  be  positive 
and should be 1.0 at a strain rate of zero.
*MAT_LOW_DENSITY_VISCOUS_FOAM 
This  is  Material  Type  73  for  Modeling  Low  Density  Urethane  Foam  with  high 
compressibility  and  with  rate  sensitivity  which  can  be  characterized  by  a  relaxation 
curve.    Its  main  applications  are  for  seat  cushions,  padding  on  the  Side  Impact 
Dummies (SID), bumpers, and interior foams.  Optionally, a tension cut-off failure can 
be defined.  Also, see the notes below and the description of material 57: *MAT_LOW_-
DENSITY_FOAM. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
LCID 
F 
5 
TC 
F 
6 
HU 
F 
7 
8 
BETA 
DAMP 
F 
F 
Default 
Remarks 
1.E+20
1. 
0.05 
3 
6 
1 
7 
8 
  Card 2 
1 
2 
3 
4 
5 
Variable 
SHAPE 
FAIL 
BVFLAG 
KCON 
LCID2 
BSTART 
TRAMP 
NV 
Type 
F 
F 
F 
F 
Default 
1.0 
0.0 
0.0 
0.0 
F 
0 
F 
F 
0.0 
0.0 
I 
6 
Relaxation  Constant  Cards.    If  LCID2 = 0  then  include  the  following  viscoelastic 
constants.    Up  to  6  cards  may  be  input.    A  keyword  card  (with  a  “*”  in  column  1) 
terminates this input if less than 6 cards are used. 
  Card 3 
Variable 
Type 
1 
GI 
F 
2 
3 
4 
5 
6 
7 
8 
BETAI 
REF 
F
Frequency  Dependence  Card.  If  LCID2 = -1  then  include  the  following  frequency 
dependent viscoelastic data. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID3 
LCID4 
SCALEW 
SCALEA 
Type 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
LCID 
TC 
HU 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s modulus used in tension.  For implicit problems E is set
to the initial slope of load curve LCID. 
Load  curve  ID,  see  *DEFINE_CURVE,  for  nominal  stress  versus 
strain. 
Tension cut-off stress 
Hysteretic  unloading  factor  between  0  and  1  (default = 1,  i.e.,  no 
energy dissipation), see also Figure M57-1 
BETA 
β, decay constant to model creep in unloading. 
EQ.0.0: No relaxation. 
DAMP 
Viscous  coefficient  (.05 < recommended  value  <.50)  to  model 
damping effects. 
LT.0.0: |DAMP|  is  the  load  curve  ID,  which  defines  the
damping constant as a function of the maximum strain
in  compression  defined  as:  𝜀max = max(1 − 𝜆1, 1 −
𝜆2, 1. −𝜆3) 
In  tension,  the  damping  constant  is  set  to  the  value  corre-
sponding  to  the  strain  at  0.    The  abscissa  should  be  defined 
from 0 to 1. 
SHAPE 
Shape  factor  for  unloading.    Active  for  nonzero  values  of  the
hysteretic  unloading  factor.    Values  less  than  one  reduces  the
energy dissipation and greater than one increases dissipation, see
also Figure M57-1.
VARIABLE   
DESCRIPTION
FAIL 
Failure option after cutoff stress is reached: 
EQ.0.0: tensile stress remains at cut-off value, 
EQ.1.0: tensile stress is reset to zero. 
BVFLAG 
Bulk viscosity activation flag, see remark below: 
EQ.0.0: no bulk viscosity (recommended), 
EQ.1.0: bulk viscosity active. 
KCON 
LCID2 
BSTART 
Stiffness  coefficient  for  contact  interface  stiffness.    Maximum
slope in stress vs.  strain curve is used.  When the maximum slope
is  taken  for  the  contact,  the  time  step  size  for  this  material  is 
reduced  for  stability.    In  some  cases  Δt  may  be  significantly 
smaller, and defining a reasonable stiffness is recommended. 
Load curve ID of relaxation curve.  If constants 𝛽𝑡  are determined 
via  a  least  squares  fit.    This  relaxation  curve  is  shown  in  Figure 
M76-1.  This model ignores the constant stress. 
Fit parameter.  In the fit, 𝛽1  is set to zero, 𝛽2  is set to BSTART, 𝛽3
is 10 times 𝛽2, 𝛽4  is 10 times greater than 𝛽3 , and so on.  If zero, 
BSTART = .01. 
TRAMP 
Optional ramp time for loading. 
NV 
Number  of  terms  in  fit.    If  zero,  the  default  is  6.    Currently,  the
maximum number is set to 6.  Values of 2 are 3 are recommended,
since  each  term  used  adds  significantly  to  the  cost.    Caution
should  be  exercised  when  taking  the  results  from  the  fit.
Preferably, all generated coefficients should be positive.  Negative
values  may  lead  to  unstable  results.    Once  a  satisfactory  fit  has
been  achieved  it  is  recommended  that  the  coefficients  which  are
written into the output file be input in future runs. 
Gi 
Optional shear relaxation modulus for the ith term 
BETAi 
Optional decay constant if ith term
REF 
*MAT_LOW_DENSITY_VISCOUS_FOAM 
DESCRIPTION
Use  reference  geometry  to  initialize  the  stress  tensor.    The
reference geometry is defined by the keyword:*INITIAL_FOAM_-
REFERENCE_GEOMETRY . 
EQ.0.0: off, 
EQ.1.0: on. 
LCID3 
LCID4 
Load  curve  ID  giving  the  magnitude  of  the  shear  modulus  as  a
function of the frequency.  LCID3 must use the same frequencies
as LCID4. 
Load curve ID giving the phase angle of the shear modulus as a
function of the frequency.  LCID4 must use the same frequencies
as LCID3. 
SCALEW 
Flag for the form of the frequency data. 
EQ.0.0: Frequency is in cycles per unit time. 
EQ.1.0: Circular frequency. 
SCALEA 
Flag for the units of the phase angle. 
EQ.0.0: Degrees. 
EQ.1.0: Radians. 
Material Formulation: 
This viscoelastic  foam model is available to model highly compressible viscous  foams.  
The hyperelastic formulation of this model follows that of Material 57.  
Rate effects are accounted for through linear viscoelasticity by a convolution integral of 
the form 
𝜎𝑖𝑗
𝑟 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)
∂𝜀𝑘𝑙
∂𝜏
𝑑𝜏
where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) is the relaxation function.  The stress tensor, 𝜎𝑖𝑗
determined  from  the  foam,  𝜎𝑖𝑗
summation of the two contributions: 
𝑟 , augments the stresses 
𝑓 ;  consequently,  the  final  stress,  𝜎𝑖𝑗,  is  taken  as  the 
𝜎𝑖𝑗 = 𝜎𝑖𝑗
𝑓 + 𝜎𝑖𝑗
𝑟 . 
Since we wish to include only simple rate effects, the relaxation function is represented 
by up to six terms of the Prony series:
𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚𝑒−𝛽𝑚𝑡
𝑚=1
This  model  is  effectively  a  Maxwell  fluid  which  consists  of  a  dampers  and  springs  in 
series.    The  formulation  is  performed  in  the  local  system  of  principal  stretches  where 
only  the  principal  values  of  stress  are  computed  and  triaxial  coupling  is  avoided.  
Consequently,  the  one-dimensional  nature  of  this  foam  material  is  unaffected  by  this 
addition  of  rate  effects.    The  addition  of  rate  effects  necessitates  42  additional  history 
variables  per  integration  point.    The  cost  and  memory  overhead  of  this  model  comes 
primarily from the need to “remember” the local system of principal stretches and the 
evaluation of the viscous stress components. 
Frequency data can be fit to the Prony series.  Using Fourier transforms the relationship 
between the relaxation function and the frequency dependent data is 
𝐺𝑠(𝜔) = 𝛼0 + ∑
𝑚=1
𝛼𝑚(𝜔/𝛽𝑚)2
1 + (𝜔/𝛽𝑚)2
𝐺ℓ(𝜔) = ∑
𝑚=1
𝛼𝑚𝜔/𝛽𝑚
1 + 𝜔/𝛽𝑚
where  the  storage  modulus  and  loss  modulus  are  defined  in  terms  of  the  frequency 
dependent  magnitude  G    and  phase  angle  𝜙  given  by  load  curves  LCID3  and  LCID4 
respectively, 
𝐺𝑠(𝜔) = 𝐺(𝜔) cos[𝜙(𝜔)]  , and 
𝐺𝑙(𝜔) = 𝐺(𝜔) sin[𝜙(𝜔)] 
Remarks: 
When hysteretic unloading is used the reloading will follow the unloading curve if the 
decay constant, β, is set to zero.  If β is nonzero the decay to the original loading curve is 
governed by the expression: 
1 − 𝑒−𝛽𝑡 
The  bulk  viscosity,  which  generates  a  rate  dependent  pressure,  may  cause  an 
unexpected volumetric response and, consequently, it is optional with this model. 
The hysteretic unloading factor results in the unloading curve to lie beneath the loading 
curve as shown in Figure M57-1.  This unloading provides energy dissipation which is 
reasonable in certain kinds of foam.
*MAT_ELASTIC_SPRING_DISCRETE_BEAM 
This  is  Material  Type  74.    This  model  permits  elastic  springs  with  damping  to  be 
combined  and  represented  with  a  discrete  beam  element  type  6.    Linear  stiffness  and 
damping  coefficients  can  be  defined,  and,  for  nonlinear  behavior,  a  force  versus 
deflection and force versus rate curves can be used.  Displacement based failure and an 
initial force are optional. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
Variable 
FLCID 
HLCID 
Type 
F 
F 
3 
K 
F 
3 
C1 
F 
4 
F0 
F 
4 
C2 
F 
5 
D 
F 
5 
6 
7 
8 
CDF 
TDF 
F 
6 
F 
7 
8 
DLE 
GLCID 
F 
I 
  VARIABLE   
DESCRIPTION
MID 
RO 
K 
F0 
D 
CDF 
TDF 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density, see also volume in *SECTION_BEAM definition. 
Stiffness coefficient. 
Optional  initial  force.    This  option  is  inactive  if  this  material  is 
referenced  in  a  part  referenced  by  material  type  *MAT_ELAS-
TIC_6DOF_SPRING 
Viscous damping coefficient. 
Compressive displacement at failure.  Input as a positive number.
After failure, no forces are carried.  This option does not apply to
zero length springs. 
EQ.0.0: inactive. 
Tensile  displacement  at  failure.    After  failure,  no  forces  are
carried.
VARIABLE   
DESCRIPTION
FLCID 
HLCID 
C1 
C2 
Load  curve  ID,  see  *DEFINE_CURVE,  defining  force  versus 
deflection for nonlinear behavior. 
Load  curve  ID,  see  *DEFINE_CURVE,  defining  force  versus 
relative velocity for nonlinear behavior (optional).  If the origin of
the  curve  is  at  (0,0)  the  force  magnitude  is  identical  for  a  given 
magnitude of the relative velocity, i.e., only the sign changes. 
Damping coefficient for nonlinear behavior (optional). 
Damping coefficient for nonlinear behavior (optional). 
DLE 
Factor to scale time units.  The default is unity. 
GLCID 
Optional  load  curve  ID,  see  *DEFINE_CURVE,  defining  a  scale 
factor versus deflection for load curve ID, HLCID.  If zero, a scale
factor of unity is assumed. 
Remarks: 
If the linear spring stiffness is used, the force, F, is given by: 
𝐹 = 𝐹0 + KΔ𝐿 + DΔ𝐿̇ 
but if the load curve ID is specified, the force is then given by: 
𝐹 = 𝐹0 + K𝑓 (Δ𝐿) {1 + C1 × Δ𝐿̇ + C2 × sgn(Δ𝐿̇)ln [max (1. ,
Δ𝐿̇
DLE
)]} + DΔ𝐿̇
+ 𝑔(Δ𝐿)ℎ(Δ𝐿̇) 
In these equations, Δ𝐿 is the change in length  
Δ𝐿 = current length − initial length 
The  cross  sectional  area  is  defined  on  the  section  card  for  the  discrete  beam  elements, 
See  *SECTION_BEAM.    The  square  root  of  this  area  is  used  as  the  contact  thickness 
offset if these elements are included in the contact treatment.
*MAT_BILKHU/DUBOIS_FOAM 
This is Material Type 75.  This model is for the simulation of isotropic crushable foams.  
Uniaxial and triaxial test data are used to describe the behavior. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
4 
5 
YM 
LCPY 
LCUYS 
F 
3 
F 
4 
F 
5 
6 
VC 
F 
6 
7 
PC 
F 
8 
VPC 
F 
7 
8 
Variable 
TSC 
VTSC 
LCRATE 
PR 
KCON 
ISFLG 
NCYCLE 
Type 
I 
F 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
YM 
LCPY 
LCUYS 
VC 
PC 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s modulus 𝐸 
Load  curve  ID  giving  pressure  for  plastic  yielding  versus
volumetric strain, see Figure M75-1. 
Load  curve  ID  giving  uniaxial  yield  stress  versus  volumetric
strain,  see Figure M75-1,  all  abscissa  values  should  be  positive  if 
only the results of a compression test are included, optionally the
results  of  a  tensile  test  can  be  added  (corresponding  to  negative
values  of  the  volumetric  strain),  in  the  latter  case  PC,  VPC,  TC
and VTC will be ignored 
Viscous  damping  coefficient  (0.05 <  recommended  value <  0.50; 
default is 0.05). 
Pressure cutoff for hydrostatic tension.  If zero, the default is  set
to  one-tenth  of  𝑝0,  the  yield  pressure  corresponding  to  a 
volumetric strain of zero.  PC will be ignored if TC is non zero.
True Stress
optional
Uniaxial Yield 
Stress (LCUYS)
Pressure Yield (LCPY)
tension
compression
Volumetric Strain 
Figure M75-1.  Behavior of crushable foam.  Unloading is elastic. 
  VARIABLE   
DESCRIPTION
VPC 
TC 
VTC 
Variable  pressure  cutoff  for  hydrostatic  tension  as  a  fraction  of
pressure  yield  value.    If  non-zero  this  will  override  the  pressure 
cutoff value PC. 
Tension  cutoff  for  uniaxial  tensile  stress.    Default  is  zero.    A
nonzero value is recommended for better stability. 
Variable  tension  cutoff  for  uniaxial  tensile  stress  as  a  fraction  of
the  uniaxial  compressive  yield  strength,  if  non-zero  this  will 
override the tension cutoff value TC. 
LCRATE 
Load curve ID giving a scale factor for the previous yield curves,
dependent upon the volumetric strain rate. 
PR 
KCON 
Poisson  coefficient,  which  applies  to  both  elastic  and  plastic
deformations, must be smaller then 0.5 
Stiffness  coefficient  for  contact  interface  stiffness.    If  undefined
one-third  of  Young’s  modulus,  YM,  is  used.    KCON  is  also
considered  in  the  element  time  step  calculation;  therefore,  large
values may reduce the element time step size.
ISFLG 
*MAT_BILKHU/DUBOIS_FOAM 
DESCRIPTION
Flag  for  tensile  response  (active  only  if  negative  abscissa  are
present in load curve LCUYS) 
EQ.0: load  curve  abscissa  in  tensile  region  correspond  to
volumetric strain 
EQ.1: load  curve  abscissa  in  tensile  region  correspond  to
effective  strain  (for  large  PR,  when  volumetric  strain 
vanishes) 
NCYCLE 
Number of cycles to determine the average volumetric strain rate.
NCYCLE is 1 by default (no smoothing) and cannot exceed 100. 
Remarks: 
The logarithmic volumetric strain is defined in terms of the relative volume, 𝑉, as: 
If option ISFLG = 1 is used, the effective strain is defined in the usual way: 
𝛾 = −ln(𝑉) 
𝜀eff = √
tr(𝛆t𝛆) 
In  defining  the  load  curve  LCPY  the  stress  and  strain  pairs  should  be  positive  values 
starting with a volumetric strain value of zero. 
The load curve LCUYS can optionally contain the results of the tensile test (correspond-
ing  to  negative  values  of  the  volumetric  strain),  if  so,  then  the  load  curve  information 
will override PC, VPC, TC and VTC. 
The yield surface is defined as an ellipse in the equivalent pressure and von Mises stress 
plane.  This ellipse is characterized by three points: 
1. 
2. 
3. 
the hydrostatic compression limit (LCPY), 
the uniaxial compression limit (LCUYS), and 
either the pressure cutoff for hydrostatic stress (PC,VPC), the tension cutoff for 
uniaxial tension (TC,VTC), or the optional tensile part of LCUYS. 
To  prevent  high  frequency  oscillations  in  the  strain  rate  from  causing  similar  high 
frequency  oscillations  in  the  yield  stress,  a  modified  volumetric  strain  rate  is  used 
obtain the scaled yield stress.  The modified strain rate is obtained as follows.  If NYCLE 
is > 1,  then  the  modified  strain  rate  is  obtained  by  a  time  average  of  the  actual  strain
rate  over  NCYCLE  solution  cycles.    The  averaged  strain  rate  is  stored  on  history 
variable #3.
*MAT_GENERAL_VISCOELASTIC_{OPTION} 
The available options include: 
<BLANK> 
MOISTURE 
This is Material Type 76.  This material model provides a general viscoelastic Maxwell 
model having up to 18 terms in the Prony series expansion and is useful for modeling 
dense  continuum  rubbers  and  solid  explosives.    Either  the  coefficients  of  the  Prony 
series  expansion  or  a  relaxation  curve  may  be  specified  to  define  the  viscoelastic 
deviatoric and bulk behavior. 
The  material  model  can  also  be  used  with  laminated  shell.    Either  an  elastic  or 
viscoelastic layer can be defined with the laminated formulation.  To activate laminated 
shell  you  need  the  laminated  formulation  flag  on  *CONTROL_SHELL.    With  the 
laminated option a user defined integration rule is needed. 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
4 
BULK 
PCF 
Type 
A8 
F 
F 
F 
5 
EF 
F 
6 
TREF 
F 
7 
A 
F 
8 
B 
F 
Relaxation Curve Card.    Leave  blank  if the  Prony  Series Cards  are  used  below.    Also, 
leave blank if an elastic layer is defined in a laminated shell. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
NT 
BSTART 
TRAMP 
LCIDK 
NTK 
BSTARTK  TRAMPK 
Type 
F 
I 
F 
F 
F 
I 
F 
F 
Moisture Card.  Additional card for MOISTURE keyword option. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MO 
ALPHA 
BETA 
GAMMA 
MST 
Type 
F 
F 
F 
F
Prony  Series  cards.    Card  Format  for  viscoelastic  constants.    Up  to  18  cards  may  be 
input.    A  keyword  card  (with  a  “*”  in  column  1)  terminates  this  input  if  less  than  18 
cards are used.  These cards are not needed if relaxation data is defined.  The number of 
terms for the shear behavior may differ from that for the bulk behavior: insert zero if a 
term  is  not  included.    If  an  elastic  layer  is  defined  you  only  need  to  define  GI  and  KI 
(note in an elastic layer only one card is needed)  
  Card 4 
Variable 
Type 
1 
GI 
F 
2 
BETAI 
F 
3 
KI 
F 
  VARIABLE   
MID 
4 
5 
6 
7 
8 
BETAKI 
F 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density. 
BULK 
Elastic bulk modulus. 
PCF 
EF 
TREF 
A 
B 
LCID 
NT 
Tensile pressure elimination flag for solid elements only.  If set to
unity tensile pressures are set to zero. 
Elastic  flag  (if  equal  1,  the  layer  is  elastic.    If  0  the  layer  is
viscoelastic). 
Reference  temperature  for  shift  function  (must  be  greater  than 
zero). 
Coefficient for the Arrhenius and the Williams-Landau-Ferry shift 
functions. 
Coefficient for the Williams-Landel-Ferry shift function. 
Load  curve  ID  for  deviatoric  relaxation  behavior.    If  LCID  is
given, constants 𝐺𝑖, and 𝛽𝑖 are determined via a least squares fit. 
See Figure M76-1 for an example relaxation curve. 
Number of terms in shear fit.  If zero the default is 6.  Fewer than
NT  terms  will  be  used  if  the  fit  produces  one  or  more  negative
shear moduli.  Currently, the maximum number is set to 18.
σ∕ε
TRAMP
10n
10n+1 10n+2 10n+3
time
optional ramp time for loading
Figure  M76-1.    Relaxation  curves  for  deviatoric  behavior  and  bulk  behavior.
The ordinate of LCID  is the deviatoric stress divided by (2 times the constant
value of deviatoric strain) where the stress and strain are in the direction of the
prescribed strain, or in non-directional terms, the effective stress divided by (3
times  the  effective  strain).    LCIDK  defines  the  mean  stress  divided  by  the
constant  value of volumetric strain imposed in a hydrostatic stress relaxation
experiment,  versus  time.    For  best  results,  the  points  defined  in  the  curve
should  be  equally  spaced  on  the  logarithmic  scale.    Note  the  values  for  the
abscissa  are  input  as  time,  not  log(time).    Furthermore,  the  curve  should  be
smooth  and  defined  in  the  positive  quadrant.    If  nonphysical  values  are
determined  by  least  squares  fit,  LS-DYNA  will  terminate  with  an  error
message  after  the  initialization  phase  is  completed.    If  the  ramp  time  for
loading is included, then the relaxation which occurs during the loading phase
is taken into account.  This effect may or may not be important. 
  VARIABLE   
BSTART 
DESCRIPTION
In the fit, 𝛽1  is set to zero, 𝛽2  is set to BSTART, 𝛽3 is 10 times 𝛽2, 
𝛽4 is 10 times 𝛽3, and so on.  If zero, BSTART is determined by an
iterative trial and error scheme. 
TRAMP 
Optional ramp time for loading. 
LCIDK 
Load  curve  ID  for  bulk  relaxation  behavior.    If  LCIDK  is  given,
constants 𝐾𝑖,  and  𝛽𝑘𝑖    are  determined  via  a  least  squares  fit.    See 
Figure M76-1 for an example relaxation curve.
VARIABLE   
NTK 
BSTARTK 
DESCRIPTION
Number  of  terms  desired  in  bulk  fit.    If  zero  the  default  is  6. 
Currently, the maximum number is set to 18. 
In  the  fit,  𝛽𝑘1,    is  set  to  zero,  𝛽𝑘2    is  set  to  BSTARTK,  𝛽𝑘3    is  10 
times 𝛽𝑘2,  𝛽𝑘4  is  100  times  greater  than 𝛽𝑘3,  and  so  on.    If  zero, 
BSTARTK is determined by an iterative trial and error scheme. 
TRAMPK 
Optional ramp time for bulk loading. 
MO 
Initial moisture, 𝑀0.  Defaults to zero. 
ALPHA 
Specifies 𝛼 as a function of moisture. 
GT.0.0:  Specifies a curve ID. 
LT.0.0:  Specifies the negative of a constant value. 
BETA 
Specifies 𝛽 as a function of moisture. 
GT.0.0:  Specifies a curve ID. 
LT.0.0:  Specifies the negative of a constant value. 
GAMMA 
Specifies 𝛾 as a function of moisture. 
GT.0.0:  Specifies a curve ID. 
LT.0.0:  Specifies the negative of a constant value. 
MST 
Moisture,  𝑀.  If  the  moisture  is  0.0,  the  moisture  option  is
disabled. 
GT.0.0:  Specifies  a  curve  ID  to  make  moisture  a  function  of
time. 
LT.0.0:  Specifies the negative of a constant value of moisture. 
GI 
Optional shear relaxation modulus for the ith term 
BETAI 
Optional shear decay constant for the ith term 
KI 
Optional bulk relaxation modulus for the ith term 
BETAKI 
Optional bulk decay constant for the ith term
*MAT_GENERAL_VISCOELASTIC 
Rate  effects  are  taken  into  accounted  through  linear  viscoelasticity  by  a  convolution 
integral of the form: 
𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)
∂𝜀𝑘𝑙
∂𝜏
𝑑𝜏
where 𝑔𝑖𝑗𝑘𝑙(𝑡−𝜏) is the relaxation functions for the different stress measures.  This stress is 
added to the stress tensor determined from the strain energy functional. 
If we wish to include only simple rate effects, the relaxation function is represented by 
18 terms from the Prony series: 
𝑔(𝑡) = ∑ 𝐺𝑚𝑒−𝛽𝑚𝑡
𝑚=1
We  characterize  this  in  the  input  by  shear  moduli,  𝐺𝑖,  and  decay  constants,  𝛽𝑖.    An 
arbitrary number of terms, up to 18, may be used when applying the viscoelastic model. 
For volumetric relaxation, the relaxation function is also represented by the Prony series 
in terms of bulk moduli: 
𝑘(𝑡) = ∑ 𝐾𝑚𝑒−𝛽𝑘𝑚𝑡
𝑚=1
The Arrhenius and Williams-Landau-Ferry (WLF) shift functions account for the effects 
of the temperature on the stress relaxation.  A scaled time, t’, 
𝑡′ = ∫ Φ(𝑇)𝑑𝑡
is  used  in  the  relaxation  function  instead  of  the  physical  time.    The  Arrhenius  shift 
function is 
Φ(𝑇) = exp [−𝐴 (
−
𝑇REF
)] 
and the Williams-Landau-Ferry shift function is 
Φ(𝑇) = exp (−𝐴
𝑇 − 𝑇REF
𝐵 + 𝑇 − 𝑇REF
) 
If  all  three  values  (TREF,  A,  and  B)  are  not  zero,  the  WLF  function  is  used;  the 
Arrhenius function is used if B is zero; and no scaling is applied if all three values are 
zero. 
The  moisture  model  allows  the  scaling  of  the  material  properties  as  a  function  of  the 
moisture content of the material.  The shear and bulk moduli are scaled by 𝛼, the decay 
constants  are  scaled  by  β,  and  a  moisture  strain,  𝛾(𝑀)[𝑀 − 𝑀𝑂]  is  introduced 
analogous to the thermal strain.
*MAT_HYPERELASTIC_RUBBER 
This  is  Material  Type  77.    This  material  model  provides  a  general  hyperelastic  rubber 
model combined optionally with linear viscoelasticity as outlined by Christensen [1980]. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
PR 
F 
4 
N 
I 
5 
NV 
I 
6 
G 
F 
7 
8 
SIGF 
REF 
F 
F 
Hysteresis Card.  Additional card read in when PR < 0 (Mullins Effect). 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TBHYS 
Type 
F 
Card 3 for N > 0.  For N > 0 a least squares fit is computed from uniaxial data. 
  Card 3 
1 
Variable 
SGL 
2 
SW 
Type 
F 
F 
3 
ST 
F 
4 
5 
6 
7 
8 
LCID1 
DATA 
LCID2 
BSTART 
TRAMP 
F 
F 
F 
F 
F 
Card 3 for N = 0.  Set the material parameters directly. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
C10 
C01 
C11 
C20 
C02 
C30 
THERML 
Type 
F 
F 
F 
F 
F 
F
Optional  Viscoelastic  Constants  &  Frictional  Damping  Constant  Cards.    Up  to  12 
cards may be input.  A keyword card (with a “*” in column 1) terminates this input if 
less than 12 cards are used.  
  Card 4 
Variable 
Type 
1 
Gi 
F 
2 
BETAi 
F 
3 
Gj 
F 
4 
5 
6 
7 
8 
SIGFj 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Poisson’s  ratio  (>  .49  is  recommended,  smaller  values  may  not
work and should not be used).  If this is set to a negative number,
then  the  absolute  value  is  used  and  an  extra  card  is  read  for
Mullins effect. 
TBHYS 
Table  ID  for  hysteresis,  could  be  positive  or  negative,  see
Remarks 1 and 2. 
N 
Number of constants to solve for: 
EQ.1: Solve for C10 and C01 
EQ.2: Solve for C10, C01, C11, C20, and C02 
EQ.3: Solve for C10, C01, C11, C20, C02, and C30 
NV 
Number  of  Prony  series  terms  in  fit.    If  zero,  the  default  is  6.
Currently, the maximum number is set to 12.  Values less than 12,
possibly  3 - 5  are  recommended,  since  each  term  used  adds
significantly  to  the  cost.    Caution  should  be  exercised  when
taking  the  results  from  the  fit. 
  Preferably,  all  generated
coefficients  should  be  positive.    Negative  values  may  lead  to
unstable  results.    Once  a  satisfactory  fit  has  been  achieved  it  is
recommended  that  the  coefficients  which  are  written  into  the
output file be input in future runs.
VARIABLE   
DESCRIPTION
G 
SIGF 
REF 
Shear  modulus  for  frequency  independent  damping.    Frequency
independent  damping  is  based  of  a  spring  and  slider  in  series.
The critical stress for the slider mechanism is SIGF defined below.
For  the  best  results,  the  value  of  G  should  be  250 - 1000  times 
greater than SIGF. 
Limit stress for frequency independent frictional damping. 
Use  reference  geometry  to  initialize  the  stress  tensor.    The
reference geometry is defined by the keyword:*INITIAL_FOAM_-
REFERENCE_GEOMETRY . 
EQ.0.0: off, 
EQ.1.0: on. 
If N>0 test information from a uniaxial test are used. 
SGL 
SW 
ST 
LCID1 
Specimen gauge length 
Specimen width 
Specimen thickness 
Load curve ID giving the force versus actual change in the gauge
length.    If  SGL,  SW,  and  ST  are  set  to  unity  (1.0),  then  curve 
LCID1 is also engineering stress versus engineering strain. 
DATA 
Type of experimental data. 
EQ.0.0: uniaxial data (Only option for this model) 
LCID2 
Load curve ID of the deviatoric stress relaxation curve, neglecting
the  long  term  deviatoric  stress.    If  LCID2  is  given,  constants  𝐺𝑖
and  𝛽𝑖  are  determined  via  a  least  squares  fit.    See  M76-1  for  an 
example  relaxation  curve.    The  ordinate  of  the  curve  is  the
viscoelastic  deviatoric  stress  divided  by  (2  times  the  constant
value  of  deviatoric  strain)  where  the  stress  and  strain  are  in  the 
direction of the prescribed strain, or in non-directional terms, the 
effective stress divided by (3 times the effective strain). 
BSTART 
In the fit, 𝛽1  is set to zero, 𝛽2  is set to BSTART, 𝛽3  is 10 times 𝛽2, 
𝛽4  is 10 times 𝛽3, and so on.  If zero, BSTART is determined by an 
iterative trial and error scheme. 
TRAMP 
Optional ramp time for loading.
VARIABLE   
DESCRIPTION
If N=0, the following constants have to be defined: 
C10 
C01 
C11 
C20 
C02 
C30 
𝐶10  
𝐶01  
𝐶11  
𝐶20  
𝐶02  
𝐶30  
THERML 
Flag for the thermal option.  If THERML > 0.0, then G, SIGF, C10 
and  C01  specify  curve  IDs  giving  the  values  as  functions  of
temperature, otherwise they specify the constants.  This option is
available only for solid elements. 
Gi 
Optional shear relaxation modulus for the ith term 
BETAi 
Optional decay constant if ith term 
Gj 
SIGFj 
Optional  shear  modulus  for  frequency  independent  damping
represented as the jth spring and slider in series in parallel to the 
rest of the stress contributions.   
Limit  stress  for  frequency  independent,  frictional,  damping
represented as the jth spring and slider in series in parallel to the 
rest of the stress contributions. 
Background: 
Rubber  is  generally  considered  to  be  fully  incompressible  since  the  bulk  modulus 
greatly  exceeds  the  shear  modulus  in  magnitude.    To  model  the  rubber  as  an 
unconstrained material a hydrostatic work term, 𝑊𝐻(𝐽), is included in the strain energy 
functional which is function of the relative volume, 𝐽, [Ogden 1984]: 
𝑊(𝐽1, 𝐽2, 𝐽) = ∑ 𝐶𝑝𝑞(𝐽1 − 3)𝑝(𝐽2 − 3)𝑞 + 𝑊𝐻(𝐽)
𝑝,𝑞=0
−1
𝐽1 = 𝐼1𝐼3
−2
𝐽2 = 𝐼2𝐼3
3⁄
3⁄
In order to prevent volumetric work from contributing to the hydrostatic work the first 
and  second  invariants  are  modified  as  shown.    This  procedure  is  described  in  more 
detail by Sussman and Bathe [1987]. 
Rate  effects  are  taken  into  account  through  linear  viscoelasticity  by  a  convolution 
integral of the form: 
𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)
∂𝜀𝑘𝑙
∂𝜏
𝑑𝜏
or in terms of the second Piola-Kirchhoff stress, 𝑆𝑖𝑗, and Green's strain tensor, 𝐸𝑖𝑗, 
𝑆𝑖𝑗 = ∫ 𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏)
∂𝐸𝑘𝑙
∂𝜏
𝑑𝜏
where  𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)  and  𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏)  are  the  relaxation  functions  for  the  different  stress 
measures.    This  stress  is  added  to  the  stress  tensor  determined  from  the  strain  energy 
functional. 
If we wish to include only simple rate effects, the relaxation function is represented by 
six terms from the Prony series: 
given by, 
𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚𝑒−𝛽𝑡
𝑚=1
𝑔(𝑡) = ∑ 𝐺𝑖𝑒−𝛽𝑖𝑡
𝑖=1
This  model  is  effectively  a  Maxwell  fluid  which  consists  of  a  dampers  and  springs  in 
series.  We  characterize this in the input by  shear moduli, 𝐺𝑖, and  decay constants,  𝛽𝑖.  
The viscoelastic behavior is optional and an arbitrary number of terms may be used.  In 
order to avoid a constant shear modulus  from this visco-elastic formulation, a term in 
the series is included only when  𝛽𝑖 > 0. 
The Mooney-Rivlin rubber model (model 27) is obtained by specifying 𝑛 = 1.  In spite of 
the  differences  in  formulations  with  model  27,  we  find  that  the  results  obtained  with 
this  model  are  nearly  identical  with  those  of  material  27  as  long  as  large  values  of 
Poisson’s ratio are used. 
The  frequency  independent  damping  is  obtained  by  the  having  a  spring  and  slider  in 
series as shown in the following sketch: 
friction
Several springs and sliders in series can be defined that are put in parallel to the rest of 
the stress contributions of this material model.
*MAT_HYPERELASTIC_RUBBER 
1.  Hysteresis  (TBHYS > 0).    If  a  positive  table  ID  for  hysteresis  is  defined,  then 
TBHYS is a table having curves that are functions of strain-energy density.  Let 
𝑊dev be the current value of the deviatoric strain energy density as calculated 
above.  Furthermore, let 𝑊̅̅̅̅̅̅dev be the peak strain energy density reached up to 
this  point  in  time.    It  is  then  assumed  that  the  resulting  stress  is  reduced  by  a 
damage factor according to 
𝐒 = 𝐷(𝑊dev, 𝑊̅̅̅̅̅̅dev)
∂𝑊dev
∂𝐄
+
∂𝑊vol
∂𝐄
. 
where 𝐷(𝑊dev, 𝑊̅̅̅̅̅̅dev) is the damage factor which is input as the table, TBHYS.  
This table consists of curves giving stress reduction (between 0 and 1) as a func-
tion of 𝑊dev indexed by 𝑊̅̅̅̅̅̅dev. 
Each 𝑊̅̅̅̅̅̅dev curve must be valid for strain energy densities between 0 and 𝑊̅̅̅̅̅̅dev.  
It is recommended that each curve be monotonically increasing, and it is required 
that  each  curve  equals  1  when  𝑊dev > 𝑊̅̅̅̅̅̅dev.    Additionally,  *DEFINE_TABLE 
requires  that  each  curve  have  the  same  beginning  and  end  point  and,  further-
more,  that  they  not  cross  except  at  the  boundaries,  although  they  are  not  re-
quired to cross. 
This table can be estimated from a uniaxial quasistatic compression test as fol-
lows: 
a)  Load the specimen to a maximum  displacement 𝑑 ̅ and measure the force 
as function of displacement: 𝑓load(𝑑 ̅). 
b)  Unload the specimen again measuring the force as a function of displace-
ment: 𝑓unload(𝑑). 
c)  The  strain  energy  density  is,  then,  given  as  a  function  of  the  loaded  dis-
placement as 
𝑊dev(𝑑) =
∫ 𝑓load(𝑠)𝑑𝑠
. 
i) 
ii) 
The peak energy, which is used to index the data set, is given by 
𝑊̅̅̅̅̅̅dev = 𝑊dev(𝑑 ̅). 
From  this  energy  curve  we  can  also  determine  the  inverse: 
𝑑(𝑊dev).  Using this inverse the load curve for LS-DYNA is then 
given by: 
𝐷(𝑊dev, 𝑊̅̅̅̅̅̅dev) =
𝑓unload[𝑑(𝑊dev)]
𝑓load[𝑑(𝑊dev)]
.
d)  This procedure is repeated for different values of 𝑑 ̅ (or equivalently 𝑊̅̅̅̅̅̅dev). 
2.  Hysteresis  (TBHYS < 0).    If  a  negative  table  ID  for  hysteresis  is  defined,  then 
all  of  the  above  holds.    The  difference  being  that  the  load  curves  comprising 
table,  |TBHYS|,  must  give  the  strain-energy  density, 𝑊dev,  as  a  function  of  the 
stress reduction factor.  This scheme guarantees that all curves have the same begin-
ning  point,  0,  and  the  same  end  point,  1.    For  negative  TBHYS  the  user  provides 
𝑊dev(𝐷, 𝑊̅̅̅̅̅̅dev) instead of 𝐷(𝑊dev, 𝑊̅̅̅̅̅̅dev).  In practice, this case corresponds to 
swapping the load curve axes.
*MAT_OGDEN_RUBBER 
This  is  also  Material  Type  77.    This  material  model  provides  the  Ogden  [1984]  rubber 
model combined optionally with linear viscoelasticity as outlined by Christensen [1980]. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
PR 
F 
4 
N 
I 
5 
NV 
I 
6 
G 
F 
7 
8 
SIGF 
REF 
F 
F 
Hysteresis Card.  Additional card read in when PR < 0 (Mullins Effect). 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TBHYS 
Type 
F 
Card 3 for N > 0.  For N > 0 a least squares fit is computed from uniaxial data. 
  Card 3 
1 
Variable 
SGL 
2 
SW 
Type 
F 
F 
3 
ST 
F 
4 
5 
6 
7 
8 
LCID1 
DATA 
LCID2 
BSTART 
TRAMP 
F 
F 
F 
F 
Card 3 for N = 0.  Set the material parameters directly. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MU1 
MU2 
MU3 
MU4 
MU5 
MU6 
MU7 
MU8 
Type 
F 
F 
F 
F 
F 
F 
F
Card 4 for N = 0.  Set the material parameters directly. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ALPHA1 
ALPHA2 
ALPHA3 
ALPHA4 
ALPHA5 
ALPHA6 
ALPHA7 
ALPHA8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Optional  Viscoelastic  Constants  Cards.    Up  to  12  cards  may  be  input.    A  keyword 
card (with a “*” in column 1) terminates this input if less than 12 cards are used. 
1 
GI 
F 
  Card 5 
Variable 
Type 
Default 
2 
3 
4 
5 
6 
7 
8 
BETAI 
VFLAG 
F 
I 
0 
  VARIABLE   
DESCRIPTION
MID 
RO 
PR 
N 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Poisson’s  ratio  (≥  49  is  recommended;  smaller  values  may  not
work and should not be used).  If this is set to a negative number,
then  the  absolute  value  is  used  and  an  extra  card  is  read  for
Mullins effect. 
Order of fit to the Ogden model, (currently < 9, 2 generally works 
okay).    The  constants  generated  during  the  fit  are  printed  in  the
output  file  and  can  be  directly  input  in  future  runs,  thereby,
saving the cost of performing the nonlinear fit.  The users need to
check  the  correction  of  the  fit  results  before  proceeding  to 
compute.
VARIABLE   
NV 
G 
SIGF 
REF 
DESCRIPTION
Number  of  Prony  series  terms  in  fit.    If  zero,  the  default  is  6.
Currently, the maximum number is set to 12.  Values less than 12,
possibly  3-5  are  recommended,  since  each  term  used  adds
significantly  to  the  cost.    Caution  should  be  exercised  when
taking  the  results  from  the  fit. 
  Preferably,  all  generated
coefficients  should  be  positive.    Negative  values  may  lead  to
unstable  results.    Once  a  satisfactory  fit  has  been  achieved  it  is
recommended  that  the  coefficients  which  are  written  into  the
output file be input in future runs. 
Shear  modulus  for  frequency  independent  damping.    Frequency
independent  damping  is  based  on  a  spring  and  slider  in  series.
The critical stress for the slider mechanism is SIGF defined below.
For  the  best  results,  the  value  of  G  should  be  250-1000  times 
greater than SIGF. 
Limit stress for frequency independent frictional damping. 
Use  reference  geometry  to  initialize  the  stress  tensor.    The
reference  geometry  is  defined  by  the  keyword:  *INITIAL_-
FOAM_REFERENCE_GEOMETRY . 
EQ.0.0: off, 
EQ.1.0: on. 
TBHYS 
Table  ID  for  hysteresis,  could  be  positive  or  negative,  see
Remarks on *MAT_HYPERELASTIC_RUBBER 
If N > 0 test information from a uniaxial test are used: 
SGL 
SW 
ST 
LCID1 
Specimen gauge length 
Specimen width 
Specimen thickness 
Load curve ID giving the force versus actual change in the gauge
length.    If  SGL,  SW,  and  ST  are  set  to  unity  (1.0),  then  curve
LCID1 is also engineering stress versus engineering strain.
VARIABLE   
DESCRIPTION
DATA 
Type of experimental data. 
EQ.1.0: uniaxial data (default) 
EQ.2.0: biaxial data 
EQ.3.0: pure shear data 
LCID2 
Load curve ID of the deviatoric stress relaxation curve, neglecting
the  long  term  deviatoric  stress.    If  LCID2  is  given,  constants  𝐺𝑖
and  𝛽𝑖  are  determined  via  a  least  squares  fit.    See  M76-1  for  an 
example  relaxation  curve.    The  ordinate  of  the  curve  is  the
viscoelastic  deviatoric  stress  divided  by  (2  times  the  constant
value  of  deviatoric  strain)  where  the  stress  and  strain  are  in  the
direction of the prescribed strain, or in non-directional terms, the 
effective stress divided by (3 times the effective strain). 
BSTART 
In the fit, 𝛽𝑖  is set to zero, 𝛽2  is set to BSTART, 𝛽3  is 10 times 𝛽2, 
𝛽4 is 10 times 𝛽3 , and so on.  If zero, BSTART is determined by an
iterative trial and error scheme. 
TRAMP 
Optional ramp time for loading. 
MUi 
𝜇𝑖, the ith shear modulus, i varies up to 8.  See discussion below. 
ALPHAi 
𝛼𝑖, the ith exponent, i varies up to 8.  See discussion below. 
Gi 
Optional shear relaxation modulus for the ith term 
BETAi 
Optional decay constant if ith term 
Flag for the viscoelasticity formulation.  This appears only on the
first  line  defining  Gi,  BETAi,  and  VFLAG.    If  VFLAG = 0,  the 
standard  viscoelasticity  formulation  is  used  (the  default),  and  if
the
viscoelasticity 
the 
VFLAG = 1, 
instantaneous elastic stress is used. 
formulation  using 
VFLAG 
Remarks: 
Rubber  is  generally  considered  to  be  fully  incompressible  since  the  bulk  modulus 
greatly  exceeds  the  shear  modulus  in  magnitude.    To  model  the  rubber  as  an 
unconstrained  material  a  hydrostatic  work  term  is  included  in  the  strain  energy 
functional which is function of the relative volume, 𝐽, [Ogden 1984]:
𝑊∗ = ∑ ∑
𝑗=1
𝑖=1
𝜇𝑗
𝛼𝑗
∗𝛼𝑗 − 1) + 𝐾(𝐽 − 1 − ln𝐽) 
(𝜆𝑖
The  asterisk  (*)  indicates  that  the  volumetric  effects  have  been  eliminated  from  the 
∗.  The number of terms, n, may vary from 1 to 8 inclusive, and 𝐾 is 
principal stretches, 𝜆𝑗
the bulk modulus. 
Rate  effects  are  taken  into  account  through  linear  viscoelasticity  by  a  convolution 
integral of the form: 
𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)
∂𝜀𝑘𝑙
∂𝜏
𝑑𝜏 
or in terms of the second Piola-Kirchhoff stress, 𝑆ij , and Green's strain tensor, 𝐸𝑖𝑗, 
𝑆𝑖𝑗 = ∫ 𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏)
∂𝐸𝑘𝑙
∂𝜏
𝑑𝜏
where  𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)  and  𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏)    are  the  relaxation  functions  for  the  different  stress 
measures.    This  stress  is  added  to  the  stress  tensor  determined  from  the  strain  energy 
functional. 
If we wish to include only simple rate effects, the relaxation function is represented by 
six terms from the Prony series: 
given by, 
𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚𝑒−𝛽𝑡
𝑚=1
𝑔(𝑡) = ∑ 𝐺𝑖𝑒−𝛽𝑖𝑡
𝑖=1
This  model  is  effectively  a  Maxwell  fluid  which  consists  of  a  dampers  and  springs  in 
series.    We  characterize  this  in  the  input  by  shear  moduli,  𝐺𝑖,  and  decay  constants, 𝛽𝑖.  
The viscoelastic behavior is optional and an arbitrary number of terms may be used.  In 
order  to  avoid  a  constant  shear  modulus  from  this  viscoelastic  formulation,  a  term  in 
the series is included only when 𝛽𝑖 > 0. 
For VFLAG = 1, the viscoelastic term is 
𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)
∂𝜎𝑘𝑙
∂𝜏
𝑑𝜏 
𝐸  is the instantaneous stress evaluated from the internal energy functional.  The 
where 𝜎𝑘𝑙
coefficients  in  the  Prony  series  therefore  correspond  to  normalized  relaxation  moduli 
instead of elastic moduli.
The Mooney-Rivlin rubber model (model 27) is obtained by specifying 𝑛 = 1.  In spite of 
the  differences  in  formulations  with  Model  27,  we  find  that  the  results  obtained  with 
this  model  are  nearly  identical  with  those  of  Material  27  as  long  as  large  values  of 
Poisson’s ratio are used. 
The  frequency  independent  damping  is  obtained  by  the  having  a  spring  and  slider  in 
series as shown in the following sketch: 
friction
*MAT_SOIL_CONCRETE 
This  is  Material  Type  78.    This  model  permits  concrete  and  soil  to  be  efficiently 
modeled.  See the explanations below. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
Variable 
1 
PC 
2 
RO 
F 
2 
OUT 
Type 
F 
F 
3 
G 
F 
3 
B 
F 
4 
K 
F 
4 
FAIL 
F 
5 
6 
7 
8 
LCPV 
LCYP 
LCFP 
LCRP 
F 
5 
F 
6 
F 
7 
F 
8 
  VARIABLE   
DESCRIPTION
MID 
RO 
G 
K 
LCPV 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Shear modulus 
Bulk modulus 
Load  curve  ID  for  pressure  versus  volumetric  strain.    The
pressure versus volumetric strain curve is defined in compression
only.    The  sign  convention  requires  that  both  pressure  and
compressive  strain  be  defined  as  positive  values  where  the
compressive  strain  is  taken  as  the  negative  value  of  the  natural
logarithm of the relative volume. 
LCYP 
Load curve ID for yield versus pressure: 
GT.0: von Mises stress versus pressure, 
LT.0:  Second  stress  invariant,  J2,  versus  pressure.    This  curve
must be defined.
1.0
Figure M78-1.  Strength reduction factor. 
  VARIABLE   
DESCRIPTION
LCFP 
LCRP 
PC 
OUT 
Load  curve  ID  for  plastic  strain  at  which  fracture  begins  versus
pressure.  This load curve ID must be defined if B > 0.0. 
Load  curve  ID  for  plastic  strain  at  which  residual  strength  is
reached  versus  pressure.    This  load  curve  ID  must  be  defined  if 
B > 0.0. 
Pressure cutoff for tensile fracture 
Output option for plastic strain in database: 
EQ.0: volumetric plastic strain, 
EQ.1: deviatoric plastic strain. 
B 
Residual strength factor after cracking, see Figure M78-1. 
FAIL 
Flag for failure: 
EQ.0: no failure, 
EQ.1: When  pressure  reaches  failure  pressure  element  is
eroded, 
EQ.2: When  pressure  reaches  failure  pressure  element  loses  it 
ability to carry tension. 
Remarks: 
Pressure  is  positive  in  compression.    Volumetric  strain  is  defined as  the  natural  log of 
the relative volume and is positive in compression where the relative volume, V, is the
*MAT_SOIL_CONCRETE 
Figure M78-2.  Cracking strain versus pressure. 
ratio of the current volume to the initial volume.  The tabulated data should be given in 
order of increasing compression.  If the pressure drops below the cutoff value specified, 
it is reset to that value and the deviatoric stress state is eliminated. 
If the load curve ID (LCYP) is provided as a positive number, the deviatoric, perfectly 
plastic, pressure dependent, yield function φ, is given as 
𝜙 = √3J2 − 𝐹(𝑝) = 𝜎𝑦 − 𝐹(𝑝) 
where  ,  F(p)  is  a  tabulated  function  of  yield  stress  versus  pressure,  and  the  second 
invariant, J2, is defined in terms of the deviatoric stress tensor as: 
𝐽2 =
𝑆𝑖𝑗𝑆𝑖𝑗 
assuming that if the ID is given as negative then the yield function becomes: 
being the deviatoric stress tensor. 
𝜙 = 𝐽2 − 𝐹(𝑝) 
If  cracking  is  invoked  by  setting  the  residual  strength  factor,  B,  on  card  2  to  a  value 
between  0.0  and  1.0,  the  yield  stress  is  multiplied  by  a  factor  f  which  reduces  with 
plastic strain according to a trilinear law as shown in Figure M78-1. 
𝑏 = residual strength factor 
1 = plastic stain at which cracking begins. 
2 = plastic stain at which residual strength is reached. 
ε1 and ε2 are tabulated functions of pressure that are defined by load curves, see Figure 
M78-2.    The  values  on  the  curves  are  pressure  versus  strain  and  should  be  entered  in 
order  of  increasing  pressure.    The  strain  values  should  always  increase  monotonically 
with pressure.
By  properly  defining  the  load  curves,  it  is  possible  to  obtain  the  desired  strength  and 
ductility over a range of pressures, see Figure M78-3. 
Yield
stress
p3
p2
p1
Figure M78-3.  Yield stress as a function of plastic strain. 
Plastic strain
*MAT_HYSTERETIC_SOIL 
This  is  Material  Type  79.    This  model  is  a  nested  surface  model  with  up  to  ten 
superposed  “layers”  of  elasto-perfectly  plastic  material,  each  with  its  own  elastic 
moduli and yield values.  Nested surface models give hysteric behavior, as the different 
“layers” yield at different stresses.  See Remarks below. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
  Card 2 
Variable 
1 
DF 
Type 
F 
  Card 3 
1 
2 
RP 
F 
2 
3 
K0 
F 
3 
4 
P0 
F 
4 
5 
B 
F 
5 
6 
A0 
F 
6 
7 
A1 
F 
7 
8 
A2 
F 
8 
LCID 
SFLC 
DIL_A 
DIL_B 
DIL_C 
DIL_D 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
GAM1 
GAM2 
GAM3 
GAM4 
GAM5 
LCD 
LCSR 
PINIT 
Type 
F 
  Card 4 
1 
F 
2 
F 
3 
F 
4 
F 
5 
I 
6 
I 
7 
I 
8 
Variable 
TAU1 
TAU2 
TAU3 
TAU4 
TAU5 
Type 
F 
F 
F 
F 
F 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density
VARIABLE   
DESCRIPTION
K0 
P0 
B 
A0 
A1 
A2 
DF 
RP 
LCID 
Bulk modulus at the reference pressure 
Cut-off/datum  pressure  (must  be  0≤  i.e.    tensile).    Below  this 
pressure, stiffness and strength disappears; this is also the “zero” 
pressure for pressure-varying properties. 
B  is  the  exponent  for  the  pressure-sensitive  elastic  moduli.    See 
remarks.  B must be in the range 0 ≤ 𝐵 < 1, and values too close 
to  1  are  not  recommended  because  the  pressure  becomes 
indeterminate. 
Yield function constant a0 (Default = 1.0), see Material Type 5. 
Yield function constant a1 (Default = 0.0), see Material Type 5. 
Yield function constant a2 (Default = 0.0), see Material Type 5. 
Damping factor.  Must be in the range 0≤df≤1: 
EQ.0:  no damping, 
EQ.1:  maximum damping. 
Reference pressure for following input data. 
Load curve ID defining shear strain verses shear stress.  Up to ten
points may be defined in the load curve.  See *DEFINE_CURVE. 
SFLD 
Scale factor to apply to shear stress in LCID. 
DIL_A 
DIL_B 
DIL_C 
DIL_D 
GAM1 
GAM2 
GAM3 
GAM4 
Dilation parameter A 
Dilation parameter B 
Dilation parameter C 
Dilation parameter D 
γ1, shear strain (ignored if LCID is non zero). 
γ2, shear strain (ignored if LCID is non zero). 
γ3, shear strain (ignored if LCID is non zero). 
γ4, shear strain (ignored if LCID is non zero).
GAM5 
LCD 
LCSR 
*MAT_HYSTERETIC_SOIL 
DESCRIPTION
γ5, shear strain (ignored if LCID is non zero). 
strain  amplitudes 
Optional  Load  Curve  ID  defining  damping  ratio  of  hysteresis  at
different 
for 
unload/reload).    The  x-axis  is  shear  strain,  the  y-axis  is  the 
damping  ratio  (e.g.,  0.05  for  5%  damping).    The  strains  (x-axis 
values) of curve LCD must be identical to those of curve LCID. 
(overrides  Masing 
rules 
Load  curve  ID  defining  plastic  strain  rate  scaling  effect  on  yield
stress.  See *DEFINE_CURVE.  The x-axis is plastic strain rate, the 
y-axis is the yield enhancement factor. 
PINIT 
Flag for pressure sensitivity (B and A0, A1, A2 equations): 
EQ.0:  Use current pressure (will vary during the analysis) 
EQ.1:  Use pressure from initial stress state 
EQ.2:  Use initial “plane stress” pressure (𝜎𝑣 + 𝜎ℎ)/2 
EQ.3:  User (compressive) initial vertical stress 
τ1, shear stress at γ1 (ignored if LCID is non zero). 
τ2, shear stress at γ2 (ignored if LCID is non zero). 
τ3, shear stress at γ3 (ignored if LCID is non zero). 
τ4, shear stress at γ4 (ignored if LCID is non zero). 
τ5, shear stress at γ5 (ignored if LCID is non zero). 
TAU1 
TAU2 
TAU3 
TAU4 
TAU5 
Remarks: 
The elastic moduli G and K are pressure sensitive: 
𝐺(𝑝) =
𝐾(𝑝) =
𝐺0(𝑝 − 𝑝0)𝑏
(𝑝ref − 𝑝0)𝑏
𝐾0(𝑝 − 𝑝0)𝑏
(𝑝ref − 𝑝0)𝑏
where G0 and K0 are the input values, p is the current pressure, p0 the cut-off or datum 
pressure (must be zero or negative).  If p attempts to fall below p0 (i.e., more tensile) the 
shear  stresses  are  set  to  zero  and  the  pressure  is  set  to  p0.    Thus,  the  material  has  no 
stiffness or strength in tension.  The pressure in compression is calculated as follows:
𝑝 = 𝑝ref [−
⁄
(1−𝑏)
𝐾0
𝑝ref
ln(𝑉)]
where V is the relative volume, i.e., the ratio between the original and current volume.  
This formula results in an instantaneous bulk modulus proportional to pb whose value 
at the reference pressure is equal to  K0/(1-b). 
The  constants  a0,  a1,  a2  govern  the  pressure  sensitivity  of  the  yield  stress.    Only  the 
ratios between these values are important - the absolute stress values are taken from the 
stress-strain curve. 
The stress strain pairs define a shear stress versus shear strain curve.  The first point on 
the curve is assumed by default to be (0,0) and does not need to be entered.  The slope 
of  the  curve  must  decrease  with  increasing  γ.    This  curves  applies  at  the  reference 
pressure; at other pressures the curve is scaled by 
𝜏(𝑝, 𝛾)
𝜏(𝑝𝑟𝑒𝑓 , 𝛾)
= √
[𝑎0 + 𝑎1(𝑝 − 𝑝0) + 𝑎2(𝑝 − 𝑝0)2]
[𝑎0 + 𝑎1(𝑝ref − 𝑝0) + 𝑎2(𝑝ref − 𝑝0)2]
The shear stress-strain curve (with points (τ1,γ1), (τ2,γ2)...(τN,γN)) is converted into a series 
of  N  elastic  perfectly-plastic  curves  such  that ∑(𝜏𝑖, (𝛾)) = 𝜏(𝛾),  as  shown  in  the  figure 
below. 
elasto-plastic 1
elasto-plastic 2
shear strain
elasto-plastic 3
elasto-plastic 4
Figure M79-1. 
low pressure
Each  elastic  perfectly-plastic  curve  represents  one  “layer”  in  the  material  model.  
Deviatoric  stresses  are  stored  and  calculated  separately  for  each  layer.    The  total
deviatoric  stress  is  the  sum  of  the  deviatoric  stresses  in  each  layer.    By  this  method, 
hysteretic  (energy-absorbing)  stress-strain  curves  are  generated  in  response  to  any 
strain cycle of amplitude greater than the lowest yield strain of any layer.  The example 
below shows response to small and large strain cycles (blue and pink lines) superposed 
on the input curve (thick red line). 
)
(
60
40
20
-20
-40
-60
backbone curve
shear strain amplitude: 0.16%
shear strain amplitude: 0.06%
-0.2
-0.1
0.1
0.2
0.3
0.4
shear strain %
Figure M79-2.  
Definition of shear strain and shear stress: 
Different  definitions  of  “shear  strain”  and  “shear  stress”  are  possible  when  applied  to 
the three-dimensional stress states.  MAT_079 uses the following definitions: 
Input shear stress is treated by the material model as, 
0.5 × Von  Mises  Stress = √(3𝜎′𝑖: 𝜎′𝑖 8⁄ ). 
Input shear strain is treated by the material model as 
1.5 × Von  Mises  Strain = √(3𝜀′𝑖: 𝜀′𝑖 2⁄ ). 
For  a  particular  stress  or  strain  state  (defined  by  the  relationship  between  the  three 
principal stresses or strains), a scaling factor may be needed in order to convert between 
the definitions given above and the shear stress or strain that an engineer would expect.  
The  MAT_079  definitions  of  shear  stress  and  shear  strain  are  derived  from  triaxial 
testing  in  which  one  principal  stress  is  applied,  while  the  other  two  principal  stresses 
are equal to a confining stress which is held constant, i.e.  principal stresses and strains
have the form (a, b, b).  If instead the user wishes the input curve to represent a test in 
which  a  pure  shear  strain  is  applied  over  a  hydrostatic  pressure,  such  as  a  shear-box 
text, then it is recommended to scale both the x-axis and the y-axis of the curve by 0.866.  
This  factor  assumes  principal  stresses  of  the  form  (p+t,  p-t,    p)  where  t  is  the  applied 
shear stress, and similar for the principal strains. 
Pressure Sensitivity: 
The  yield  stresses  of  the  layers,  and  hence  the  stress  at  each  point  on  the  shear  stress-
strain  input  curve,  vary  with  pressure  according  to  constants  A0,  A1  and  A2.    The 
elastic moduli, and hence also the slope of each section of shear stress-strain curve, vary 
with  pressure  according  to  constant  B.    These  effects  combine  to  modify  the  shear 
stress-strain curve according to pressure: 
1 ≠ θ
2, slope
varies with pressure
according to B
stress varies
with pressure
according to
A0, A1, and A2
at different P, same point on
the input stress-strain curve
will be reached at different strain
high pressure (P2)
low pressure (P1)
shear strain
Figure M79-3. 
Pressure sensitivity can make the solution sensitive to numerical noise.  In cases where 
the  expected  pressure changes  are  small  compared  to  the  initial  stress  state,  it  may  be 
preferable to use pressure from the initial stress state instead of current pressure as the 
basis  for  the  pressure  sensitivity  (option  PINIT).    This  causes  the  bulk  modulus  and 
shear  stress-strain  curve  to  be  calculated  once  for  each  element  at  the  start  of  the 
analysis and to remain fixed thereafter.  PINIT affects both stiffness (calculated using B) 
and  strength  (calculated  using  A0,  A1  and  A2).    If  PINIT  options  2  (“plane  stress” 
pressure) or 3 (vertical stress) are used, these quantities substitute for pressure p in the 
equations above.  Input values of pref and p0 should then also be “plane stress” pressure 
or vertical stress, respectively.
If  PINIT  is  used,  B  is  allowed  to  be  as  high  as  1.0  (stiffness  proportional  to  initial 
pressure); otherwise, values of B higher than about 0.5 are not recommended. 
Dilatancy: 
Parameters DIL_A, DIL_B, DIL_C and DIL_D control the compaction and dilatancy that 
occur  in  sandy  soils  as  a  result  of  shearing  motion.    The  dilatancy  is  expressed  as  a 
volume strain γv: 
𝜀v = 𝜀r + 𝜀g 
𝜀r = DIL_ A(Γ)DIL_ B 
𝜀g =
∫(𝑑𝛾𝑥𝑧
2⁄
2 )
2 + 𝑑𝛾𝑦𝑧
DIL_ C + DIL_ D × ∫(𝑑𝛾𝑥𝑧
2⁄
2 )
2 + 𝑑𝛾𝑦𝑧
Γ = (𝛾𝑥𝑧
2⁄  
2 )
2 + 𝛾𝑦𝑧
𝛾𝑥𝑧 = 2𝜀𝑥𝑧 
𝛾𝑦𝑧 = 2𝜀𝑦𝑧 
γr  describes  the  dilation  of  the  soil  due  to  the  magnitude  of  the  shear  strains;  this  is 
caused by the soil particles having to climb over each other to develop shear strain. 
γg describes compaction of the soil due to collapse of weak areas and voids, caused by 
continuous shear straining. 
Recommended inputs for sandy soil: 
DIL_A 
DIL_B 
DIL_C 
DIL_D 
-  10 
-  1.6 
-  100 
-  2.5 
DIL_A and DIL_B may cause instabilities in some models.   If this  facility is  used  with 
pore water pressure, liquefaction can be modeled. 
Strain rate sensitivity: 
Strain  rate  effect  is  accounted  for  by  scaling  the  yield  stress  of  each  layer  as  the  user-
specified  function  of  plastic  strain  rate.    The  stress-strain  curve  defined  by  LCID  is 
considered as the reference curve or the curve for the lowest shear strength among all 
plastic  strain  rates.    Scale  factor  versus  strain  rate  is  defined  in  curve  LCSR.    All  scale 
factors must be equal to or larger than 1.0.  For a given plastic strain rate, the effective 
scale factor for the resultant stress (instead of layer stresses) is 1.0 for elastic range and
ramping up to the one corresponding to the given plastic strain rate when the stress is 
approaching the ultimate yield stress (last point of curve LCID).
*MAT_RAMBERG-OSGOOD 
This is Material Type 80.  This model is intended as a simple model of shear behavior 
and can be used in seismic analysis. 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
4 
5 
GAMY 
TAUY 
ALPHA 
Type 
A8 
F 
F 
F 
F 
6 
R 
F 
7 
8 
BULK 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density. 
GAMY 
TAUY 
Reference shear strain (γy) 
Reference shear stress (τy) 
ALPHA 
Stress coefficient (α) 
R 
Stress exponent (r) 
BULK 
Elastic bulk modulus 
Remarks: 
The  Ramberg-Osgood  equation  is  an  empirical  constitutive  relation  to  represent  the 
one-dimensional elastic-plastic behavior of many materials, including soils.  This model 
allows  a  simple  rate  independent  representation  of  the  hysteretic  energy  dissipation 
observed  in  soils  subjected  to  cyclic  shear  deformation.    For  monotonic  loading,  the 
stress-strain relationship is given by:  
𝛾𝑦
𝛾𝑦
=
=
𝜏𝑦
𝜏𝑦
∣
∣
+ 𝛼 ∣
𝜏𝑦
− 𝛼 ∣
𝜏𝑦
,  for 𝛾 ≥ 0 
,  for 𝛾 < 0
where 𝛾 is the shear and 𝜏 is the stress.  The model approaches perfect plasticity as the 
stress  exponent  𝑟 → ∞.    These  equations  must  be  augmented  to  correctly  model 
unloading  and  reloading  material  behavior.    The  first  load  reversal  is  detected  by 
𝛾𝛾̇ < 0.  After the first reversal, the stress-strain relationship is modified to 
(𝛾 − 𝛾0)
2𝛾𝑦
(𝛾 − 𝛾0)
2𝛾𝑦
=
=
(𝜏 − 𝜏0)
2𝜏𝑦
(𝜏 − 𝜏0)
2𝜏𝑦
+ 𝛼 ∣
− 𝛼 ∣
′
(𝜏 − 𝜏0)
∣
2𝜏𝑦
′
(𝜏 − 𝜏0)
∣
2𝜏𝑦
,  for 𝛾 ≥ 0
,  for 𝛾 < 0
where 𝛾0 and 𝜏0 represent the values of strain and stress at the point of load reversal.  
Subsequent load reversals are detected by (𝛾 − 𝛾0)𝛾̇ < 0. 
The  Ramberg-Osgood  equations  are  inherently  one-dimensional  and  are  assumed  to 
apply to shear components.  To generalize this theory to the multidimensional case, it is 
assumed that each component of the deviatoric stress and deviatoric tensorial strain is 
independently  related  by  the  one-dimensional  stress-strain  equations.    A  projection  is 
used  to  map  the  result  back  into  deviatoric  stress  space  if  required.    The  volumetric 
behavior is elastic, and, therefore, the pressure p is found by 
where 𝜀𝑣 is the volumetric strain.
𝑝 = −𝐾𝜀𝑣
*MAT_PLASTICITY_WITH_DAMAGE_{OPTION} 
This manual entry apply to both types 81 and 82.  Materials 81 and 82 model an elasto-
visco-plastic  material  with  user-defined  isotropic  stress  versus  strain  curves,  which, 
themselves,  may  be  strain-rate  dependent.    This  model  accounts  for  the  effects  of 
damage  prior  to  rupture  based  on  an  effective  plastic-strain  measure.    Additionally, 
failure can be triggered when the time step drops below some specified value. 
Available options include: 
<BLANK> 
ORTHO 
ORTHO_RCDC 
ORTHO_RCDC1980 
STOCHAS 
The ORTHO option invokes an orthotropic damage model, an extension that was first 
added as for modelling failure in aluminum panels.  Directional damage begins after a 
defined  failure  strain  is  reached  in  tension  and  continues  to  evolve  until  a  tensile 
rupture strain is reached in either one of the two orthogonal directions.  After rupture is 
detected at all integration points, the element is deleted.   
The ORTHO_RCDC option invokes the damage model developed by Wilkins [Wilkins, 
et al.  1977].  The ORTHO_RCDC1980 option invokes a damage model based on strain 
invariants  as  developed  by  Wilkins  [Wilkins,  et  al.    1980].    A  nonlocal  formulation, 
which  requires  additional  storage,  is  used  if  a  characteristic  length  is  defined.    The 
RCDC  option,  which  was  added  at  the  request  of  Toyota,  works  well  in  predicting 
failure in cast aluminum; see Yamasaki, et al., [2006]. 
NOTE:  This  keyword,  in  its  long  form,  *MAT_PLASTICI-
TY_WITH_DAMAGE,  with  no  options  invokes  ma-
terial type 81.  Adding an orthotropic damage option 
will  invoke  material  type  82.    Since  type  82  must 
track  directional  strains  it  is,  computationally,  more 
expensive.
Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
6 
7 
8 
SIGY 
ETAN 
EPPF 
TDEL 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
0.0 
1012 
0.0 
  Card 2 
Variable 
Type 
Default 
1 
C 
F 
0 
  Card 3 
1 
2 
P 
F 
0 
2 
3 
4 
5 
LCSS 
LCSR 
EPPFR 
F 
0 
3 
F 
0 
4 
F 
1014 
5 
6 
VP 
F 
0 
6 
7 
8 
LCDM 
NUMINT 
F 
0 
7 
I 
0 
8 
Variable 
EPS1 
EPS2 
EPS3 
EPS4 
EPS5 
EPS6 
EPS7 
EPS8 
Type 
Default 
F 
0 
  Card 4 
1 
F 
0 
2 
F 
0 
3 
F 
0 
4 
F 
0 
5 
F 
0 
6 
F 
0 
7 
F 
0 
8 
Variable 
ES1 
ES2 
ES3 
ES4 
ES5 
ES6 
ES7 
ES8 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F
Ortho RCDC Card.  Additional card for keyword option ORTHO_RCDC. 
  Card 5 
1 
2 
3 
4 
Variable 
ALPHA 
BETA 
GAMMA 
D0 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
5 
B 
F 
0 
6 
7 
LAMBDA 
DS 
F 
0 
F 
0 
8 
L 
F 
0 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
SIGY 
ETAN 
EPPF 
TDEL 
C 
P 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
Yield stress. 
Tangent modulus, ignored if (LCSS.GT.0) is defined. 
𝜀failure
, effective plastic strain at which material softening begins. 
Minimum time step size for automatic element deletion. 
Strain rate parameter, 𝐶, see formula below. 
Strain rate parameter, 𝑃, see formula below. 
LCSS 
Load curve ID or Table ID. 
1.  Case 1: LCSS is a load curve ID.  The load curve LCSS maps 
effective  plastic  strain  to  effective  stress.    If  the  fields
EPS1 - EPS8 and ES1 - ES8 are defined, they are ignored. 
2.  Case  2:  LCSS  is  a  Table  ID.    Each  strain  rate  value  is 
associated to a load curve ID giving the stress as a func-
tion  of  effective  plastic  strain  for  that  rate,  See  Figure 
M24-1.  The stress versus effective plastic strain curve for
the  lowest  value  of  strain  rate  is  used  if  the  strain  rate
falls  below  the  minimum  value.    Likewise,  the  stress
VARIABLE   
DESCRIPTION
versus  effective  plastic  strain  curve  for  the  highest  value
of  strain  rate  is  used  if  the  strain  rate  exceeds  the  maxi-
mum  value.    The  strain  rate  parameters:  C  and  P;  the
curve ID, LCSR; EPS1 - EPS8 and ES1 - ES8 are ignored if 
a Table ID is defined. 
The  strain  rate  values  defined  in  the  table  may  be  given
as  the  natural  logarithm  of  the  strain  rate.    If  the  first
stress-strain  curve  in  the  table  corresponds  to  a  negative
strain rate, LS-DYNA assumes that the natural logarithm 
of the strain rate value is used.  Since the tables are inter-
nally  discretized  to  equally  space  the  points,  natural
logarithms are necessary, for example, if the curves corre-
spond to rates from 10−4 to 104. 
LCSR 
Load curve ID defining strain rate scaling effect on yield stress. 
EPPFR 
𝜀rupture
, effective plastic strain at which material ruptures. 
VP 
Formulation for rate effects: 
EQ.0.0: Scale yield stress (default), 
EQ.1.0: Viscoplastic formulation. 
LCDM 
NUMINT 
Optional curve ID defining nonlinear damage curve.  To activate
the  damage  curve  either  the  EPPF  or  EPPFR  fields  must  contain
nonzero values. 
Number  of  through  thickness  integration  points  which  must  fail
before  a  shell  element  is  deleted.    (If  zero,  all  points  must  fail.) 
The  default  of  all  integration  points  is  not  recommended  since
shells undergoing large strain are often not deleted due to nodal
fiber rotations which limit strains at active integration points after
most points have failed.  Better results are obtained if NUMINT is 
set to 1 or a number less than one half of the number of through
thickness  points.    For  example,  if  four  through  thickness  points
are used, NUMINT should not exceed 2, even for fully integrated
shells which have 16 integration points. 
EPS1 - EPS8 
Effective  plastic  strain  values  (optional  if  SIGY  is  defined).    At
least 2 points should be defined. 
ES1 - ES8 
Corresponding yield stress values to EPS1 - EPS8.
yield stress versus
effective plastic strain
for undamaged material
failure begins
nominal stress
after failure
damage, ω, increases
linearly with plastic
strain after failure
rupture
Figure M81-1.  Stress strain behavior when damage is included 
  VARIABLE   
DESCRIPTION
ALPHA 
Parameter 𝛼. for the Rc-Dc model 
BETA 
Parameter 𝛽. for the Rc-Dc model 
GAMMA 
Parameter 𝛾. for the Rc-Dc model 
D0 
B 
Parameter 𝐷0. for the Rc-Dc model 
Parameter 𝑏. for the Rc-Dc model 
LAMBDA 
Parameter 𝜆. for the Rc-Dc model 
Parameter 𝐷𝑠. for the Rc-Dc model 
Optional  characteristic  element  length  for  this  material.    We
recommend  that  the  default  of  0  always  be  used,  especially  in
parallel  runs.    If  zero,  nodal  values  of  the  damage  function  are
used to compute the damage gradient.  See discussion below. 
DS 
L 
Remarks: 
The  stress  strain  behavior  may  be  treated  by  a  bilinear  stress  strain  curve  by  defining 
the tangent modulus, ETAN.  Alternately, a curve similar to that shown in Figure M24-1
is  expected  to  be  defined  by  (EPS1,  ES1)  -  (EPS8,  ES8);  however,  an  effective  stress 
versus  effective  plastic  strain  curve  (LCSS)  may  be  input  instead  if  eight  points  are 
insufficient.    The  cost  is  roughly  the  same  for  either  approach.    The  most  general 
approach is to use the table definition (LCSS) discussed below. 
Three options to account for strain rate effects are possible: 
1.  Strain rate may be accounted for using the Cowper and Symonds model which 
scales the yield stress with the factor 
1 + (
6⁄
)
𝜀̇
where 𝜀̇ is the strain rate, 𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗. 
If the viscoplastic option is active, VP = 1.0, and if SIGY is > 0 then the dynamic 
𝑝 ),  which  is 
yield  stress  is  computed  from  the  sum  of  the  static  stress,  𝜎𝑦
typically given by a load curve ID, and the initial yield stress, SIGY, multiplied 
by the Cowper-Symonds rate term as follows: 
𝑠(𝜀eff
𝜎𝑦(𝜀eff
𝑝 , 𝜀̇eff
𝑝 ) = 𝜎𝑦
𝑠(𝜀eff
𝑝 ) + SIGY ×
𝑝⁄
𝜀̇eff
⎟⎞
𝐶 ⎠
⎜⎛
⎝
where  the  plastic  strain  rate  is  used.    With  this  latter  approach  similar  results 
can be obtained between this model and material model: *MAT_ANISOTROP-
IC_VISCOPLASTIC.  If SIGY = 0, the following equation is used instead where 
𝑝 ), must be defined by a load curve: 
the static stress, 𝜎𝑦
𝑠(𝜀eff
𝜎𝑦(𝜀eff
𝑝 , 𝜀̇eff
𝑝 ) = 𝜎𝑦
𝑝 )
𝑠(𝜀eff
𝜀̇eff
⎟⎞
𝐶 ⎠
⎜⎛
⎝
⎡
1 +
⎢⎢
⎣
𝑝⁄
⎤
⎥⎥
⎦
This latter equation is always used if the viscoplastic option is off. 
2.  For  complete  generality  a  load  curve  (LCSR)  to  scale  the  yield  stress  may  be 
input instead.  In this curve the scale factor versus strain rate is defined. 
3. 
If different stress versus strain curves can be provided for various strain rates, 
the  option  using  the  reference  to  a  table  (LCSS)  can  be  used.    Then  the  table 
input in *DEFINE_TABLE is expected, see Figure M24-1. 
The constitutive properties for the damaged material are obtained from the undamaged 
material properties.  The amount of damage evolved is represented by the constant, 𝜔, 
which varies from zero if no damage has occurred to unity for complete rupture.  For 
uniaxial loading, the nominal stress in the damaged material is given by  
𝜎nominal =
failure
Figure M81-2.  A nonlinear damage curve is optional.  Note that the origin of
the curve is at (0,0).  It is permissible to input the failure strain EPPF as zero for
this option.  The nonlinear damage curve is useful for controlling the softening
behavior after the failure strain is reached. 
where P is the applied load and A is the surface area.  The true stress is given by:  
where 𝐴loss is the void area.  The damage variable can then be defined: 
𝜎true =
𝐴 − 𝐴loss
such that 
𝜔 =
𝐴loss
0 ≤ 𝜔 ≤ 1. 
In  this  model,  unless  LCDM  is  defined  by  the  user,  damage  is  defined  in  terms  of 
effective plastic strain after the failure strain is exceeded as follows: 
𝑝 − 𝜀failure
𝜀eff
− 𝜀failure
𝜀rupture
𝑝 ≤ 𝜀rupture
𝜀failure
≤ 𝜀eff
𝜔 =
,
After exceeding the failure strain softening begins and continues until the rupture strain 
is reached. 
The Rc-Dc model is defined as: 
The damage D is given by 
where 𝜀𝑝 is the effective plastic strain,  
𝐷 = ∫ 𝜔1𝜔2𝑑𝜀𝑝 
𝜔1 = (
1 − 𝛾𝜎m
)
is a triaxial stress weighting term and 
𝜔2 = (2 − 𝐴𝐷)𝛽 
is a asymmetric strain weighting term.  In the above 𝜎m is the mean stress.  For 𝐴𝐷 we 
use  
𝐴𝐷 = min (∣
𝜎2
𝜎3
∣ , ∣
𝜎3
𝜎2
∣) 
where  𝜎𝑖  are  the  principal  stresses  and  𝜎1 > 𝜎2 > 𝜎3.    Fracture  is  initiated  when  the 
accumulation of damage is 
where 𝐷𝑐 is the a critical damage given by 
𝐷𝑐
> 1 
A fracture fraction,  
𝐷𝑐 = 𝐷0(1 + 𝑏|∇𝐷|𝜆) 
𝐹 =
𝐷 − 𝐷𝑐
𝐷𝑠
defines the degradations of the material by the Rc-Dc model. 
For  the  Rc-Dc  model  the  gradient  of  damage  needs  to  be  estimated.    The  damage  is 
connected to the integration points, and, thus, the computation of the gradient requires 
some  manipulation  of  the  LS-DYNA  source  code.    Provided  that  the  damage  is 
connected to nodes, it can be seen as a standard bilinear field and the gradient is easily 
obtained.    To  enable  this,  the  damage  at  the  integration  points  are  transferred  to  the 
nodes  as  follows.    Let  𝐸𝑛  be  the  set  of  elements  sharing  node  𝑛,  𝐸𝑛  the  number  of 
elements in that set, 𝑃𝑒 the set of integration points in element 𝑒 and ∣𝑃𝑒∣ the number of 
points in that set.  The average damage 𝐷̅̅̅̅̅ 𝑒 in element 𝑒 is computed as  
𝐷̅̅̅̅̅ 𝑒 =
∑ 𝐷𝑝
𝑝∈𝑃𝑒
∣𝑃𝑒∣
where 𝐷𝑝 is the damage  in integration point 𝑝. Finally, the damage value in  node 𝑛 is 
estimated as 
𝐷𝑛 =
∑ 𝐷̅̅̅̅̅ 𝑒
𝑒∈𝐸𝑛
|𝐸𝑛|
. 
This  computation  is  performed  in  each  time  step  and  requires  additional  storage.  
Currently we use three times the total number of nodes in the model for this calculation, 
but  this  could  be  reduced  by  a  considerable  factor  if  necessary.    There  is  an  Rc-Dc 
option for the Gurson dilatational-plastic model.  In the implementation of this model, 
𝑙   be  the  set  of  elements  from 
the  norm  of  the  gradient  is  computed  differently.    Let  𝐸𝑓
𝑙 ∣  be  the 
within  a  distance  𝑙  of  element,  𝑓   not  including  the  element  itself,  and  let  ∣𝐸𝑓
number  of  elements  in  that  set.    The  norm  of  the  gradient  of  damage  is  estimated 
roughly as 
‖∇𝐷‖𝑓 ≈
𝑙 ∣
∣𝐸𝑓
∑
𝑒∈𝐸𝑓
∣𝐷𝑒 − 𝐷𝑓 ∣
𝑑𝑒𝑓
where 𝑑𝑒𝑓  is the distance between element 𝑓  and 𝑒. 
The  reason  for  taking  the  first  approach  is  that  it  should  be  a  better  approximation  of 
the gradient, it can for one integration point in each element be seen as a weak gradient 
of an elementwise constant field.  The memory consumption as well as computational 
work should not be much higher than for the other approach. 
The RCDC1980 model is identical to the RCDC model except the expression for 𝐴𝐷is in 
terms of the principal stress deviators and takes the form 
𝐴𝐷 = max (∣
𝑆2
𝑆3
∣ , ∣
𝑆2
𝑆1
∣) 
The STOCHASTIC option allows spatially varying yield and failure behavior.  See *DE-
FINE_STOCHASTIC_VARIATION for additional information. 
*DEFINE_MATERIAL_HISTORIES Properties 
Label 
Attributes 
Description 
Instability 
Plastic Strain Rate 
Damage 
- 
- 
- 
- 
- 
- 
- 
- 
- 
- 
- 
𝑝 , see EPPF 
Failure indicator 𝜀eff
𝑝  
Effective plastic strain rate 𝜀̇eff
𝑝 /𝜀fail
-  Damage 𝜔
*MAT_FU_CHANG_FOAM_{OPTION} 
This is Material Type 83. 
Available options include: 
DAMAGE_DECAY 
LOG_LOG_INTERPOLATION 
Rate  effects  can  be  modeled  in  low  and  medium  density  foams,  see  Figure  M83-1.  
Hysteretic unloading behavior in this model is a function of the rate sensitivity with the 
most rate sensitive foams providing the largest hysteresis and vice versa.  The unified 
constitutive  equations  for  foam  materials  by  Chang  [1995]  provide  the  basis  for  this 
model.    The  mathematical  description  given  below  is  excerpted  from  the  reference.  
Further  improvements  have  been  incorporated  based  on  work  by  Hirth,  Du  Bois,  and 
Weimar [1998].  Their improvements permit: load curves generated by drop tower test 
to  be  directly  input,  a  choice  of  principal  or  volumetric  strain  rates,  load  curves  to  be 
defined in tension, and the volumetric behavior to be specified by a load curve.  
The unloading response was generalized by Kolling, Hirth, Erhart and Du Bois [2006] to 
allow  the  Mullin’s  effect  to  be  modeled,  i.e.,  after  the  first  loading  and  unloading, 
further reloading occurs on the unloading curve.  If it is desired to reload on the loading 
curves  with  the  new  generalized  unloading,  the  DAMAGE  decay  option  is  available 
which  allows  the  reloading  to  quickly  return  to  the  loading  curve  as  the  damage 
parameter decays back to zero in tension and compression. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
KCON 
F 
5 
TC 
F 
6 
7 
8 
FAIL 
DAMP 
TBID 
F 
F 
F 
Default 
none 
none 
none 
none 
1.E+20 
none 
0.05 
none 
Remarks
> > > ε
tensile
Optional Tensile Behavior
TFLAG = 1
compressive
Nominal Strain
Default Tensile Behavior
TFLAG = 0
Figure  M83-1.    Rate  effects  in  the  nominal  stress  versus  engineering  strain
curves, which are used to model rate effects in Fu Chang’s foam model. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
Variable 
BVFLAG 
SFLAG 
RFLAG 
TFLAG 
PVID 
SRAF 
REF 
Type 
F 
F 
F 
F 
F 
F 
F 
8 
HU 
F 
Default 
1.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Remarks 
1 
2 
3 
4
Card 3 for DAMAGE_DECAY keyword option.  
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MINR 
MAXR 
SHAPE 
BETAT 
BETAC 
Type 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
Card 3 for keyword option NOT set to DAMAGE_DECAY. 
  Card 3 
Variable 
1 
D0 
Type 
F 
2 
N0 
F 
3 
N1 
F 
4 
N2 
F 
5 
N3 
F 
6 
C0 
F 
7 
C1 
F 
8 
C2 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Card 4 for  keyword option NOT set to DAMAGE_DECAY. 
  Card 4 
Variable 
1 
C3 
Type 
F 
2 
C4 
F 
3 
C5 
F 
4 
AIJ 
5 
SIJ 
6 
7 
8 
MINR 
MAXR 
SHAPE 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0
*MAT_FU_CHANG_FOAM 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EXPON 
RIULD 
Type 
F 
F 
Default 
1.0 
0.0 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
KCON 
TC 
FAIL 
DAMP 
TBID 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s modulus 
Optional  Young's  modulus  used  in  the  computation  of  sound
speed.  This will influence the time step, contact forces, hourglass
stabilization forces, and the numerical damping (DAMP). 
EQ.0.0: KCON is set equal to the, 
max(𝐸, current tangent to stresss-strain curve), 
if  TBID ≠ 0.    Otherwise,  if  TBID = 0,  KCON  is  set 
equal to the maximum slope of the stress-strain curve. 
Tension cut-off stress 
Failure option after cutoff stress is reached: 
EQ.0.0: tensile stress remains at cut-off value, 
EQ.1.0: tensile stress is reset to zero. 
Viscous 
(0.05 < recommended value < 0.50; default is 0.05). 
coefficient 
model 
to 
damping 
effects
Table ID, see *DEFINE_TABLE, for nominal stress vs.  strain data 
as a function of strain rate.  If the table ID is provided, cards 3 and
4 may be left blank and the fit will be done internally.  The Table
ID can be positive or negative .  If TBID < 0, 
enter |TBID| on the *DEFINE_TABLE keyword.
VARIABLE   
DESCRIPTION
BVFLAG 
Bulk viscosity activation flag, see Remark 1: 
EQ.0.0: no bulk viscosity (recommended), 
EQ.1.0: bulk viscosity active. 
SFLAG 
Strain rate flag : 
EQ.0.0: true constant strain rate, 
EQ.1.0: engineering strain rate. 
RFLAG 
Strain rate evaluation flag see Remark 3: 
EQ.0.0: first principal direction, 
EQ.1.0: principal strain rates for each principal direction, 
EQ.2.0: volumetric strain rate. 
TFLAG 
Tensile stress evaluation: 
EQ.0.0: linear in tension. 
EQ.1.0: input  via  load  curves  with  the  tensile  response
corresponds to negative values of stress and strain. 
PVID 
Optional  load  curve  ID  defining  pressure  versus  volumetric
strain.  See Remark 4. 
SRAF 
Strain rate averaging flag.  See Remark 5.  
LT.0.0:  use exponential moving average. 
EQ.0.0: use weighted running average. 
EQ.1.0: average the last twelve values. 
REF 
HU 
D0 
Use  reference  geometry  to  initialize  the  stress  tensor.    The 
reference  geometry  is  defined  by  the  keyword:  *INITIAL_-
FOAM_REFERENCE_GEOMETRY . 
EQ.0.0: off, 
EQ.1.0: on. 
Hysteretic  unloading  factor  between  0  and  1  (default = 0).    See 
also Remark 6 and Figure M83-4. 
material constant, see equations below.
VARIABLE   
N0 
N1 
N2 
N3 
C0 
C1 
C2 
C3 
C4 
C5 
AIJ, 
SIJ 
DESCRIPTION
material constant, see equations below. 
material constant, see equations below. 
material constant, see equations below. 
material constant, see equations below. 
material constant, see equations below. 
material constant, see equations below. 
material constant, see equations below. 
material constant, see equations below. 
material constant, see equations below. 
material constant, see equations below. 
material constant, see equations below. 
material constant, see equations below. 
MINR 
Ratemin, minimum strain rate of interest. 
MAXR 
Ratemax, maximum strain rate of interest. 
SHAPE 
BETAT 
BETAC 
EXPON 
Shape  factor  for  unloading.    Active  for  nonzero  values  of  the
hysteretic unloading factor HU.  Values less than one reduces the
energy dissipation and greater than one increases dissipation, see
also Figure M83-2. 
Decay constant for damage in tension.  The damage decays after
loading in ceases according to 𝑒−BETAT×𝑡. 
Decay constant for damage in compression.  The damage decays
after loading in ceases according to 𝑒−BETAC×𝑡. 
Exponent  for  unloading.    Active  for  nonzero  values  of  the
hysteretic unloading factor HU.  Default is 1.0 
RIULD 
Flag for rate independent unloading, see Remark 6.   
EQ.0.0: off, 
EQ.1.0: on.
*MAT_083 
The strain is divided into two parts: a linear part and a non-linear part of the strain 
and the strain rate becomes 
𝐄(𝑡) = 𝐄𝐿(𝑡) + 𝐄𝑁(𝑡) 
𝐄̇(𝑡) = 𝐄̇𝐿(𝑡) + 𝐄̇𝑁(𝑡) 
where 𝐄̇𝑁 is an expression for the past history of 𝐄𝑁.  A postulated constitutive equation 
may be written as: 
∞
𝛔(𝑡) = ∫ [𝐄𝑡
𝑁(𝜏), 𝐒(𝑡)]
𝑑𝜏 
where 𝐒(𝑡) is the state variable and ∫
∞ and  
𝜏=0
∞
.𝜏=0 is a functional of all values of 𝜏 in 𝑇𝜏: 0 ≤ 𝜏 ≤
𝑁(𝜏) = 𝐄𝑁(𝑡 − 𝜏) 
𝐄𝑡
where 𝜏 is the history parameter: 
𝑁(𝜏 = ∞) ⇔ the virgin material 
𝐄𝑡
It is assumed that the material remembers only its immediate past, i.e., a neighborhood 
about 𝜏 = 0.  Therefore, an expansion of 𝐄𝑡
𝑁(𝜏) in a Taylor series about 𝜏 = 0 yields:
𝑁(𝜏) = 𝐄𝑁(0) +
𝐄𝑡
∂𝐄𝑡
∂𝑡
(0)𝑑𝑡 
Hence, the postulated constitutive equation becomes: 
𝛔(𝑡) = 𝛔∗[𝐄𝑁(𝑡), 𝐄̇𝑁(𝑡), 𝐒(𝑡)] 
where we have replaced 
∂𝐄𝑡
∂𝑡  by 𝐄̇𝑁, and 𝛔∗ is a function of its arguments. 
For a special case, 
we may write 
𝛔(𝑡) = 𝛔∗(𝐄𝑁(𝑡), 𝐒(𝑡)) 
𝐄̇
𝑁 = 𝑓 (𝐒(𝑡), 𝐬(𝑡)) 
which  states  that  the nonlinear  strain  rate  is  the  function  of  stress  and  a  state  variable 
which  represents  the  history  of  loading.    Therefore,  the  proposed  kinetic  equation  for 
foam materials is: 
𝐄̇
𝑁 =
‖𝛔‖
𝐷0exp {−𝑐0 [
𝛔: 𝐒
(‖𝛔‖)2]
2𝑛0
}
where 𝐷0, 𝑐0, and 𝑛0 are material constants, and 𝐒 is the overall state variable.  If either 
𝐷0 = 0 or 𝑐0 → ∞ then the nonlinear strain rate vanishes. 
𝑆̇𝑖𝑗 = [𝑐1(𝑎𝑖𝑗𝑅 − 𝑐2𝑆𝑖𝑗)𝑃 + 𝑐3𝑊𝑛1(∥𝐄̇𝑁∥)𝑛2𝐼𝑖𝑗]𝑅 
𝑛3
∥𝐄̇𝑁∥
𝑐5
− 1]
𝑅 = 1 + 𝑐4 [
𝑃 = 𝛔: 𝐄̇𝑁 
𝑊 = ∫ 𝛔: (𝑑𝐄) 
where c1, c2, c3, c4, c5, n1, n2, n3, and aij are material constants and: 
2 
‖𝛔‖ = (𝜎𝑖𝑗𝜎𝑖𝑗)
∥𝐄̇∥ = (𝐸̇𝑖𝑗𝐸̇𝑖𝑗)
2 
∥𝐄̇𝑁∥ = (𝐸̇𝑁
𝑖𝑗𝐸̇𝑁
2 
𝑖𝑗)
In  the  implementation  by  Fu  Chang  the  model  was  simplified  such  that  the  input 
constants 𝑎𝑖𝑗 and the state variables 𝑆𝑖𝑗 are scalars. 
Additional Remarks: 
1.  Bulk Viscosity.  The bulk viscosity, which generates a rate dependent pressure, 
may cause an unexpected volumetric response and consequently, it is optional 
with this model. 
2.  Constant Velocity Loading.  Dynamic  compression tests at the strain rates of 
interest in vehicle crash are usually performed with a drop tower.  In this test 
the  loading  velocity  is  nearly  constant  but  the  true  strain  rate,  which  depends 
on  the  instantaneous  specimen  thickness,  is  not.    Therefore,  the  engineering 
strain rate input is optional so that the stress strain curves obtained at constant 
velocity loading can be used directly.  See the SFLAG field.
> >
Current State
Nominal Strain
Figure M83-2.  HU=0, TBID>0 
3.  Strain Rates with Multiaxial Loading.  To further improve the response under 
multiaxial loading, the strain rate parameter can either be based on the princi-
pal strain rates or the volumetric strain rate.  See the RFLAG field. 
4.  Triaxial  Loading.    Correlation  under  triaxial  loading  is  achieved  by  directly 
inputting  the  results  of  hydrostatic  testing  in  addition  to  the  uniaxial  data.  
Without  this  additional  information  which  is  fully  optional,  triaxial  response 
tends to be underestimated.  See the PVID field. 
5.  Strain  Rate  Averaging.    Three  different  options  are  available.    The  default, 
SRAF = 0.0,  uses  a  weighted  running  average  with  a  weight  of  1/12  on  the 
current  strain  rate.    With  the  second  option,  SRAF = 1.0,  the  last  twelve  strain 
rates  are  averaged.    The  third  option,  SRAF < 0,  uses  an  exponential  moving 
average  with  factor  |SRAF|  representing  the  degree  of  weighting  decrease 
(−1 ≤ SRAF < 0).  The averaged strain rate at time 𝑡𝑛 is obtained by: 
averaged = |SRAF|𝜀̇𝑛 + (1 − |SRAF|)𝜀̇𝑛−1
𝜀̇𝑛
averaged 
6.  Unloading  Response  Options.    Several  options  are  available  to  control 
unloading response in MAT_083: 
a)  HU = 0 and TBID > 0.  See Figure M83-2. 
This is the old way.  In this case the unloading response will follow the 
curve  with  the  lowest  strain  rate  and  is  rate-independent.    The  curve 
with lowest strain rate value (typically zero) in TBID should correspond 
to  the  unloading  path  of  the  material  as  measured  in  a  quasistatic  test.
> > > ε
Current State
Nominal Strain
Figure M83-3.  HU = 0, TBID < 0 
The quasistatic loading path then corresponds to a realistic (small) value 
of the strain rate. 
b)  HU = 0 and TBID < 0 
In  this  case  the  curve  with  lowest  strain  rate  value  (typically  zero)  in 
TBID  must  correspond  to  the  unloading  path  of  the  material  as  meas-
ured in a quasistatic test.  The quasistatic loading path then corresponds 
to a realistic (small) value of the strain rate.  At least three curves should 
be  used  in  the  table  (one  for  unloading,  one  for  quasistatic,  and  one  or 
more  for  dynamic  response).    The  quasistatic  loading  and  unloading 
path  (thus  the  first  two  curves  of  the  table)  should  form  a  closed  loop.  
The unloading response is given by a damage formulation for the prin-
cipal stresses as follows: 
𝜎𝑖 = (1 − 𝑑)𝜎𝑖 
The damage parameter d is computed internally in such a way that the 
unloading path under uniaxial tension and compression is fitted exactly 
in the simulation.  The unloading response is rate dependent in this case.  
In some cases, this rate dependence for loading and unloading can lead 
to noisy results.  To reduce that noise, it is possible to switch to rate in-
dependent unloading with RIULD = 1.
> > > ε
Current State
Unloading curve computed
internally based on HU and SHAPE
Nominal Strain
Figure M83-4.  HU > 0, TBID > 0 
c)  HU > 0 and TBID > 0 
No unloading curve should be provided in the table and the curve with 
the  lowest  strain  rate  value  in  TBID  should  correspond  to  the  loading 
path of the material as measured in a quasistatic test.  At least two curves 
should be used in the table (one for quasistatic and one or more for dy-
namic response).  In this case the unloading response is given by a dam-
age formulation for the principal stresses as follows: 
𝜎𝑖 = (1 − 𝑑)𝜎𝑖 
𝑑 = (1 − 𝐻𝑈)
⎢⎡1 − (
⎣
𝑊cur
𝑊max
SHAPE
EXPON
)
⎥⎤
⎦
where W corresponds to the current value of the hyperelastic energy per 
unit undeformed volume.  The unloading response is rate dependent in 
this case.  In some cases, this rate dependence for loading and unloading 
can lead to noisy results.  To reduce that noise, it is possible to switch to 
rate independent unloading with RIULD = 1. 
The LOG_LOG_INTERPOLATION option uses log-log interpolation for 
table TBID in the strain rate direction.
*MAT_WINFRITH_CONCRETE 
This  is  Material  Type  84  with  optional  rate  effects.    The  Winfrith  concrete  model  is  a 
smeared crack (sometimes known as pseudo crack), smeared rebar model, implemented 
in  the  8-node  single  integration  point  continuum  element,  i.e.,  ELFORM = 1  in  *SEC-
TION_SOLID.    It  is  recommended  that  a  double  precision  executable  be  used  when 
using this material model.  Single precision may produce unstable results. 
This model  was developed by Broadhouse and Neilson [1987], and Broadhouse [1995] 
over  many  years  and  has  been  validated  against  experiments.    The  input  documenta-
tion  given  here  is  taken  directly  form  the  report  by  Broadhouse.    The  Fortran 
subroutines  and  quality  assurance  test  problems  were  also  provided  to  LSTC  by  the 
Winfrith Technology Center.   
Rebar  may  be  defined  using  the  command  *MAT_WINFRITH_CONCRETE_REIN-
FORCEMENT which appears in the following section. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
  Card 2 
Variable 
Type 
1 
E 
F 
  Card 3 
1 
2 
YS 
F 
2 
3 
TM 
F 
3 
4 
PR 
F 
4 
5 
6 
UCS 
UTS 
F 
5 
F 
6 
7 
FE 
F 
7 
8 
ASIZE 
F 
8 
EH 
UELONG 
RATE 
CONM 
CONL 
CONT 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
EPS1 
EPS2 
EPS3 
EPS4 
EPS5 
EPS6 
EPS7 
EPS8 
Type 
F 
F 
F 
F 
F 
F 
F
Card 4 
Variable 
1 
P1 
Type 
F 
2 
P2 
F 
3 
P3 
F 
4 
P4 
F 
5 
P5 
F 
6 
P6 
F 
7 
P7 
F 
8 
P8 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
TM 
PR 
UCS 
UTS 
FE 
Material identification.  A unique number or label not exceeding
8 characters must be specified. 
Mass density. 
Initial tangent modulus of concrete. 
Poisson's ratio. 
Uniaxial compressive strength. 
Uniaxial tensile strength. 
Depends on value of RATE below. 
RATE.EQ.0: Fracture  energy  (energy  per  unit  area  dissipated
in opening crack). 
RATE.EQ.1: Crack  width  at  which  crack-normal  tensile  stress 
goes to zero. 
ASIZE 
Aggregate size (radius). 
E 
YS 
EH 
Young's modulus of rebar. 
Yield stress of rebar. 
Hardening modulus of rebar 
UEONG 
Ultimate elongation before rebar fails.
RATE 
Rate effects: 
*MAT_WINFRITH_CONCRETE 
DESCRIPTION
EQ.0.0: Strain  rate  effects  are  included.    WARNING:  energy
may not be conserved using this option. 
EQ.1.0: Strain  rate  effects  are  turned  off.    Crack  widths  are
stored as extra history variables 30, 31, 32. 
EQ.2.0:  Like RATE = 1 but includes improved crack algorithm 
(recommended).  Crack widths are stored as extra his-
tory variables 3, 4, 5. 
CONM 
GT.0:  Factor to convert model mass units to kg. 
EQ.-1.:  Mass,  length,  time  units  in  model  are  lbf ×  sec2/in, 
inch, sec. 
EQ.-2.:  Mass, length, time units in model are g, cm, microsec.
EQ.-3.:  Mass, length, time units in model are g, mm, msec. 
EQ.-4.:  Mass, length, time units in model are metric ton, mm, 
sec. 
EQ.-5.:  Mass, length, time units in model are kg, mm, msec. 
CONL 
CONM.GT.0:  CONL  is  the  conversion  factor  from  model
length units to meters. 
CONM.LE.0:  CONL is ignored. 
CONT 
CONM.GT.0: CONL  is  the  conversion  factor  from  time  units 
to seconds 
CONM.LE.0:  CONT is ignored. 
EPS1, EPS2, … 
Volumetric  strain  values  (natural  logarithmic  values),  see
Remarks below.  A maximum of 8 values are allowed.   
P1, P2, … 
Pressures  corresponding  to  volumetric  strain  values  given  on
Card 3. 
Remarks: 
Pressure is positive in compression; volumetric strain is given by the natural log of the 
relative volume and is negative in compression.  The tabulated data are given in order 
of increasing compression, with no initial zero point.
If the volume compaction curve is omitted, the following scaled curve is automatically 
used where 𝑝1 is the pressure at uniaxial compressive failure from: 
𝑝1 =
𝜎𝑐
and 𝐾 is the bulk unloading modulus computed from 
𝐾 =
𝐸𝑠
3(1 − 2𝑣)
where 𝐸𝑠 is the input tangent modulus for concrete and 𝑣 is Poisson's ratio. 
Volumetric Strain
Pressure
−𝑝1/𝐾
−0.002
−0.004
−0.010
−0.020
−0.030
−0.041
−0.051
−0.062
−0.094
1.00𝑝1
1.50𝑝1
3.00𝑝1
4.80𝑝1
6.00𝑝1
7.50𝑝1
9.45𝑝1
11.55𝑝1
14.25𝑝1
25.05𝑝1
Table  M84-1.    Default  pressure  versus  volumetric  strain 
curve for concrete if the curve is not defined. 
The  Winfrith  concrete  model  can  generate  an  additional  binary  output  database 
containing information on crack locations, directions, and widths.  In order to generate 
the crack database, the LS-DYNA execution line is modified by adding: 
where crf is the desired name of the crack database, e.g., q=d3crack. 
q=crf 
LS-PrePost  can  display  the  cracks  on  the  deformed  mesh  plots.    To  do  so,  read  the 
d3plot  database  into  LS-PrePost  and  then  select  File  →  Open  →  Crack  from  the  top 
menu  bar.    Or,  open  the  crack  database  by  adding  the  following  to  the  LS-PrePost 
execution line: 
where crf is the name of the crack database, e.g., q=d3crack. 
q=crf 
By  default,  all  the  cracks  in  visible  elements  are  shown.    You  can  eliminate  narrow 
cracks from the display by setting a minimum crack width for displayed cracks.  Do this
by choosing Settings → Post Settings → Concrete Crack Width.  From the top menu bar 
of LS-PrePost, choosing Misc → Model Info  will reveal the number of cracked elements 
and the maximum crack width in a given plot state.  
An  ASCII  “aea_crack”  output  file  is  written  if  the  command  *DATABASE_BINARY_-
D3CRACK command is included in the input deck.  This command does not have any 
bearing on the aforementioned binary crack database.
*MAT_WINFRITH_CONCRETE_REINFORCEMENT 
This  is  *MAT_084_REINF  for  rebar  reinforcement  supplemental  to  concrete  defined 
using Material type 84.  Reinforcement may be defined in specific  groups of elements, 
but it is usually more convenient to define a two-dimensional mat in a specified layer of 
a  specified  material.    Reinforcement  quantity  is  defined  as  the  ratio  of  the  cross-
sectional  area of  steel relative  to the  cross-sectional  area  of  concrete  in  the  element  (or 
layer).    These  cards  may  follow  either  one  of  two  formats  below  and  may  also  be 
defined in any order. 
Option 1 (Reinforcement quantities in element groups). 
  Card 1 
1 
2 
3 
Variable 
EID1 
EID2 
INC 
Type 
I 
I 
I 
4 
XR 
F 
5 
YR 
F 
6 
ZR 
F 
7 
8 
Option 2 (Two dimensional layers by part ID).  Option 2 is active when first entry is left 
blank. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
AXIS 
COOR 
RQA 
RQB 
Type 
blank 
I 
I 
F 
F 
F 
  VARIABLE   
DESCRIPTION
EID1 
EID2 
INC 
XR 
YR 
ZR 
First element ID in group. 
Last element ID in group 
Element increment for generation. 
𝑥-reinforcement  quantity  (for  bars  running  parallel  to  global  𝑥-
axis). 
𝑦-reinforcement  quantity  (for  bars  running  parallel  to  global  𝑦-
axis). 
𝑧-reinforcement  quantity  (for  bars  running  parallel  to  global  𝑧-
axis).
VARIABLE   
PID 
DESCRIPTION
Part  ID  of  reinforced  elements.    If  PID = 0,  the  reinforcement  is 
applied to all parts which use the Winfrith concrete model. 
AXIS 
Axis normal to layer. 
EQ.1: A and B are parallel to global 𝑦 and 𝑧, respectively. 
EQ.2: A and B are parallel to global 𝑥 and 𝑧, respectively. 
EQ.3: A and B are parallel to global 𝑥 and 𝑦, respectively. 
COOR 
Coordinate location of layer: 
AXIS.EQ.1: 𝑥-coordinate 
AXIS.EQ.2: 𝑦-coordinate 
AXIS.EQ.3: 𝑧-coordinate 
RQA 
RQB 
Reinforcement quantity (A). 
Reinforcement quantity (B). 
Remarks: 
1.  Reinforcement quantity is the ratio of area of reinforcement in an element to the 
element's total cross-sectional area in a given direction.  This definition is true 
for both Options 1 and 2.  Where the options differ is in the manner in which it 
is decided which elements are reinforced.  In Option 1, the reinforced element 
IDs  are  spelled  out.    In  Option  2,  elements  of  part  ID  PID  which  are  cut  by  a 
plane (layer) defined by AXIS and COOR are reinforced.
*MAT_ORTHOTROPIC_VISCOELASTIC 
This  is  Material  Type  86.    It  allows  the  definition  of  an  orthotropic  material  with  a 
viscoelastic part.  This model applies to shell elements. 
NOTE: This material does not support specification of a ma-
terial  angle,  𝛽𝑖,  for  each  through-thickness  integra-
tion point of a shell. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
Variable 
1 
G0 
Type 
F 
  Card 3 
1 
2 
RO 
F 
2 
3 
EA 
F 
3 
4 
EB 
F 
4 
5 
EC 
F 
5 
6 
VF 
F 
6 
7 
K 
F 
7 
8 
8 
GINF 
BETA 
PRBA 
PRCA 
PRCB 
F 
2 
F 
3 
F 
4 
F 
5 
Variable 
GAB 
GBC 
GCA 
AOPT 
MANGLE 
Type 
F 
  Card 4 
1 
F 
2 
F 
3 
Variable 
Type 
F 
F 
4 
A1 
F 
5 
A2 
F 
7 
8 
7 
8 
F 
6 
6 
A3
Variable 
1 
V1 
Type 
F 
  VARIABLE   
MID 
*MAT_ORTHOTROPIC_VISCOELASTIC 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
7 
8 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
EA 
EB 
EC 
VF 
K 
G0 
GINF 
BETA 
PRBA 
PRCA 
PRCB 
GAB 
GBC 
GCA 
AOPT 
Mass density 
Young’s Modulus 𝐸𝑎 
Young’s Modulus 𝐸𝑏 
Young’s Modulus 𝐸𝑐 
Volume fraction of viscoelastic material 
Elastic bulk modulus 
𝐺0, short-time shear modulus 
𝐺∞, long-time shear modulus 
𝛽, decay constant 
Poisson’s ratio, 𝜈𝑏𝑎
Poisson’s ratio, 𝜈𝑐𝑎 
Poisson’s ratio, 𝜈𝑐𝑏 
Shear modulus, 𝐺𝑎𝑏 
Shear modulus, 𝐺𝑏𝑐 
Shear modulus, 𝐺𝑐𝑎 
Material  axes  option  : 
EQ.0.0:  locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
VARIABLE   
DESCRIPTION
NATE_NODES,  and  then  rotated  about  the  shell  ele-
ment normal by an angle MANGLE. 
EQ.2.0:  globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_ECTOR. 
EQ.3.0:  locally  orthotropic  material  axes  determined  by 
rotating the material axes about the element normal by
an angle, MANGLE, from a line in the plane of the el-
ement defined by the cross product of the vector 𝐯 with 
the element normal. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID 
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
MANGLE 
Material angle in degrees for AOPT = 0 and 3, may be overridden 
on the element card, see *ELEMENT_SHELL_BETA. 
A1 A2 A3 
Define components of vector 𝐚 for AOPT = 2. 
V1 V2 V3 
Define components of vector 𝐯 for AOPT = 3. 
D1 D2 D3 
Define components of vector 𝐝 for AOPT = 2. 
Remarks: 
For the orthotropic definition it is referred to Material Type 2 and 21.
*MAT_CELLULAR_RUBBER 
This  is  Material  Type  87.    This  material  model  provides  a  cellular  rubber  model  with 
confined  air  pressure  combined  with  linear  viscoelasticity  as  outlined  by  Christensen 
[1980].  See Figure M87-1. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
PR 
F 
4 
N 
I 
5 
6 
7 
8 
Card 2 if N > 0, a least squares fit is computed from uniaxial data  
  Card 2 
1 
Variable 
SGL 
2 
SW 
Type 
F 
F 
3 
ST 
F 
4 
5 
6 
7 
8 
LCID 
F 
Card 2 if N = 0, define the following constants  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
C10 
C01 
C11 
C20 
C02 
Type 
F 
  Card 3 
Variable 
1 
P0 
F 
2 
PHI 
F 
3 
IVS 
Type 
F 
F 
F 
  VARIABLE   
MID 
6 
7 
8 
F 
4 
G 
F 
F 
5 
BETA 
F 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density
VARIABLE   
DESCRIPTION
PR 
N 
Poisson’s  ratio,  typical  values  are  between  .0  to  .2.    Due  to  the
large  compressibility  of  air,  large  values  of  Poisson’s  ratio
generates physically meaningless results. 
Order  of  fit  (currently < 3).    If  n > 0  then  a  least  square  fit  is 
computed  with  uniaxial  data.    The  parameters  given  on  card  2
should  be  specified.    Also  see  *MAT_MOONEY_RIVLIN_RUB-
BER  (material  model  27).    A  Poisson’s  ratio  of  .5  is  assumed  for
the  void  free  rubber  during  the  fit.      The  Poisson’s  ratio  defined
on Card 1 is for the cellular rubber.  A void fraction formulation is 
used. 
Define, if N > 0: 
SGL 
SW 
ST 
LCID 
Define, if N = 0: 
C10 
C01 
C11 
C20 
C02 
P0 
PHI 
IVS 
G 
Specimen gauge length l0 
Specimen width 
Specimen thickness 
Load  curve  ID  giving  the  force  versus  actual  change  ΔL  in  the 
gauge length.  If SGL, SW, and ST are set to unity (1.0), then curve
LCID is also engineering stress versus engineering strain. 
Coefficient, C10 
Coefficient, C01 
Coefficient, C11 
Coefficient, C20 
Coefficient, C02 
Initial air pressure, P0 
Ratio of cellular rubber to rubber density, Φ 
Initial volumetric strain, γ
0 
Optional shear relaxation modulus, 𝐺, for rate effects (viscosity) 
BETA 
Optional decay constant, 𝛽1
Rubber Block with Entrapped Air
Air
Figure  M87-1.  Cellular  rubber  with  entrapped  air.    By  setting  the  initial  air
pressure to zero, an open cell, cellular rubber can be simulated. 
Remarks: 
Rubber  is  generally  considered  to  be  fully  incompressible  since  the  bulk  modulus 
greatly  exceeds  the  shear  modulus  in  magnitude.    To  model  the  rubber  as  an 
unconstrained material a hydrostatic work term, 𝑊𝐻(𝐽), is included in the strain energy 
functional which is function of the relative volume, 𝐽, [Ogden 1984]: 
𝑊(𝐽1, 𝐽2, 𝐽) = ∑ 𝐶𝑝𝑞(𝐽1 − 3)𝑝
𝑝,𝑞=0
(𝐽2 − 3)𝑞 + 𝑊𝐻(𝐽) 
𝐽1 + 𝐼1𝐼3
𝐽2 + 𝐼2𝐼3
−1
3⁄  
−2
3⁄  
In order to prevent volumetric work from contributing to the hydrostatic work the first 
and  second  invariants  are  modified  as  shown.    This  procedure  is  described  in  more 
detail by Sussman and Bathe [1987]. 
The effects of confined air pressure in its overall response characteristics is included by 
augmenting the stress state within the element by the air pressure. 
𝜎𝑖𝑗 = 𝜎𝑖𝑗
𝑠𝑘 − 𝛿𝑖𝑗𝜎 air 
𝑠𝑘  is  the  bulk  skeletal  stress  and  𝜎 𝑎𝑖𝑟  is  the  air  pressure  computed  from  the 
where  𝜎𝑖𝑗
equation:
𝜎 air = −
𝑝0𝛾
1 + 𝛾 − 𝜙
where  p0  is  the  initial  foam  pressure  usually  taken  as  the  atmospheric  pressure  and  γ 
defines the volumetric strain  
𝛾 = 𝑉 − 1 + 𝛾0 
where V is the relative volume of the voids and γ0 is the initial volumetric strain which 
is typically zero.  The rubber skeletal material is assumed to be incompressible. 
Rate  effects  are  taken  into  account  through  linear  viscoelasticity  by  a  convolution 
integral of the form: 
𝜎𝑖𝑗 = ∫ 𝑔 𝑖𝑗𝑘𝑙
(𝑡 − 𝜏)
∂𝜀𝑘𝑙
∂𝜏
𝑑𝜏
or in terms of the second Piola-Kirchhoff stress, 𝑆𝑖𝑗, and Green's strain tensor, 𝐸𝑖𝑗, 
𝑆𝑖𝑗 = ∫ 𝐺 𝑖𝑗𝑘𝑙
(𝑡 − 𝜏)
∂𝜀𝑘𝑙
∂𝜏
𝑑𝜏
(𝑡 − 𝜏)  and  𝐺 𝑖𝑗𝑘𝑙
where  𝑔 𝑖𝑗𝑘𝑙
measures.    This  stress  is  added  to  the  stress  tensor  determined  from  the  strain  energy 
functional. 
(𝑡 − 𝜏)are  the  relaxation  functions  for  the  different  stress 
Since we wish to include only simple rate effects, the relaxation function is represented 
by one term from the Prony series: 
𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚𝑒−𝛽𝑡
𝑚=1
given by, 
𝑔(𝑡) = 𝐸𝑑𝑒−𝛽1𝑡. 
This  model  is  effectively  a  Maxwell  fluid  which  consists  of  a  damper  and  spring  in 
series.  We characterize this in the input by a shear modulus, 𝐺, and decay constant, 𝛽1. 
The Mooney-Rivlin rubber model (model 27) is obtained by specifying n = 1 without air 
pressure  and  viscosity.    In  spite  of  the  differences  in  formulations  with  Model  27,  we 
find that the results obtained with this model are nearly identical with those of material 
type 27 as long as large values of Poisson’s ratio are used.
*MAT_MTS 
This is Material Type 88.  The MTS model is due to Mauldin, Davidson, and Henninger 
[1990] and is available for applications involving large strains, high pressures and strain 
rates.    As  described  in  the  foregoing  reference,  this  model  is  based  on  dislocation 
mechanics  and  provides  a  better  understanding  of  the  plastic  deformation  process  for 
ductile materials by using an internal state variable call the mechanical threshold stress.  
This  kinematic  quantity  tracks  the  evolution  of  the  material’s  microstructure  along 
some arbitrary strain, strain rate, and temperature-dependent path using a differential 
form that balances dislocation generation and recovery processes.  Given a value for the 
mechanical  threshold  stress,  the  flow  stress  is  determined  using  either  a  thermal-
activation-controlled or a drag-controlled kinetics relationship.  An equation-of-state is 
required  for  solid  elements  and  a  bulk  modulus  must  be  defined  below  for  shell 
elements. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
4 
5 
6 
7 
8 
SIGA 
SIGI 
SIGS 
SIG0 
BULK 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
8 
Variable 
HF0 
HF1 
HF2 
SIGS0 
EDOTS0 
BURG 
CAPA 
BOLTZ 
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
SM0 
SM1 
SM2 
EDOT0 
GO 
PINV 
QINV 
EDOTI 
Type 
F 
  Card 4 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
G0I 
PINVI 
QINVI 
EDOTS 
G0S 
PINVS 
QINVS 
Type 
F 
F 
F 
F 
F 
F
Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RHOCPR 
TEMPRF 
ALPHA 
EPS0 
Type 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
SIGA 
SIGI 
SIGS 
SIG0 
HF0 
HF1 
HF2 
SIGS0 
BULK 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
𝜎̂𝑎, dislocation interactions with long-range barriers (force/area). 
𝜎̂𝑖, dislocation interactions with interstitial atoms (force/area).
𝜎̂𝑠, dislocation interactions with solute atoms (force/area).
𝜎̂0, initial value of 𝜎̂  at zero plastic strain (force/area) NOT USED.
𝑎0, dislocation generation material constant (force/area).
𝑎1, dislocation generation material constant (force/area).
𝑎2, dislocation generation material constant (force/area).
𝜎̂εso, saturation threshold stress at 0o K (force/area).
Bulk  modulus  defined  for  shell  elements  only.    Do  not  input  for
solid elements.
EDOTS0 
𝜀̇εso, reference strain-rate (time-1). 
BURG 
Magnitude  of  Burgers  vector 
(distance)
(interatomic  slip  distance),
CAPA 
Material constant, A. 
BOLTZ 
Boltzmann’s constant, k (energy/degree). 
SM0 
SM1 
𝐺0, shear modulus at zero degrees Kelvin (force/area). 
𝑏1, shear modulus constant (force/area).
DESCRIPTION
*MAT_MTS 
SM2 
𝑏2, shear modulus constant (degree).
EDOT0 
𝜀̇𝑜, reference strain-rate (time-1).
G0 
PINV 
QINV 
𝑔0,  normalized  activation  energy  for  a  dislocation/dislocation
interaction.
𝑝, material constant. 
𝑞, material constant. 
EDOTI 
𝜀̇𝑜,𝑖, reference strain-rate (time-1). 
G0I 
PINVI 
QINVI 
𝑔0,𝑖,  normalized  activation  energy  for  a  dislocation/interstitial
interaction.
𝑝𝑖
𝑞𝑖
, material constant.
, material constant. 
EDOTS 
𝜀̇𝑜,𝑠, reference strain-rate (time-1). 
G0S 
PINVS 
QINVS 
𝑔0,𝑠  normalized  activation  energy  for  a  dislocation/solute
interaction.
𝑝𝑠
𝑞𝑠
, material constant.
, material constant. 
RHOCPR 
𝜌𝑐𝑝, product of density and specific heat. 
TEMPRF 
𝑇ref, initial element temperature in degrees K.
ALPHA 
𝛼, material constant (typical value is between 0 and 2).
EPS0 
𝜀𝑜, factor to normalize strain rate in the calculation of Θ𝑜. (time-1).
Remarks: 
The flow stress 𝜎 is given by: 
𝜎 = 𝜎̂𝑎 +
𝐺0
[𝑠th𝜎̂ + 𝑠th,𝑖𝜎̂𝑖 + 𝑠th,𝑠𝜎̂𝑠]
The  first  product  in  the  equation  for  𝜏  contains  a  micro-structure  evolution  variable, 
i.e.,𝜎̂ ,  called  the  Mechanical  Threshold  Stress    (MTS),  that  is  multiplied  by  a  constant-
structure  deformation  variable  s𝑡ℎ: s𝑡ℎ  is  a  function  of  absolute  temperature  T  and  the 
plastic  strain-rates  𝜀̇p.    The  evolution  equation  for  𝜎̂   is  a  differential  hardening  law 
representing dislocation-dislocation interactions: 
∂
∂𝜀𝑝 ≡ Θ𝑜
⎡
⎢⎢
1 −
⎢
⎣
tanh (𝛼 𝜎̂
𝜎̂𝜀𝑠
tanh(𝛼)
)
⎤
⎥⎥
⎥
⎦
The  term,  ∂𝜎̂
∂𝜀𝑝,  represents  the  hardening  due  to  dislocation  generation  and  the  stress 
ratio,  𝜎̂
, represents softening due to dislocation recovery.  The threshold stress at zero 
𝜎̂𝜀𝑠
strain-hardening 𝜎̂𝜀𝑠 is called the saturation threshold stress.  Relationships for Θ𝑜, 𝜎̂𝜀𝑠 
are: 
Θ𝑜 = 𝑎𝑜 + 𝑎1ln (
𝜀̇𝑝
𝜀0
) + 𝑎2√
𝜀̇𝑝
𝜀0
which contains the material constants, 𝑎𝑜, 𝑎1, and 𝑎2.  The constant, 𝜎̂𝜀𝑠, is given as: 
𝜎̂εs = 𝜎̂εso (
𝑘𝑇/𝐺𝑏3𝐴
)
𝜀̇𝑝
𝜀̇εso
which  contains  the  input  constants:  𝜎̂𝜀𝑠𝑜,  𝜀̇𝜀𝑠𝑜,  𝑏,  A,  and  k.    The  shear  modulus  G 
appearing in these equations is assumed to be a function of temperature and is given by 
the correlation. 
𝐺 = 𝐺0 − 𝑏1 (𝑒𝑏2 𝑇⁄ − 1)
⁄
which  contains  the  constants:  𝐺0,  𝑏1,  and  𝑏2.    For  thermal-activation  controlled 
deformation 𝑠𝑡ℎ is evaluated via an Arrhenius rate equation of the form: 
⎧
{{{
⎨
{{{
⎩
The absolute temperature is given as: 
𝑠𝑡ℎ =
1 −
⎡𝑘𝑇ln (
⎢⎢⎢
⎣
𝐺𝑏3𝑔0
𝜀̇0
𝜀̇𝑝)
⎤
⎥⎥⎥
⎦
⎫
}}}
⎬
}}}
⎭
where E is the internal energy density per unit initial volume.
𝑇 = 𝑇ref +
𝜌𝑐𝑝
*MAT_PLASTICITY_POLYMER 
This  is  Material  Type  89.    An  elasto-plastic  material  with  an  arbitrary  stress  versus 
strain  curve  and  arbitrary  strain  rate  dependency  can  be  defined.    It  is  intended  for 
applications  where  the  elastic  and  plastic  sections  of  the  response  are  not  as  clearly 
distinguishable  as  they  are  for  metals.    Rate  dependency  of  failure  strain  is  included.  
Many polymers show a more brittle response at high rates of strain. 
5 
6 
7 
8 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
Default 
none 
none 
none 
none 
  Card 2 
Variable 
Type 
Default 
1 
C 
F 
0 
  Card 3 
1 
2 
P 
F 
0 
2 
3 
4 
5 
6 
7 
8 
LCSS 
LCSR 
F 
0 
3 
F 
0 
4 
5 
6 
7 
8 
Variable 
EFTX 
DAMP 
RFAC 
LCFAIL 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density.
VARIABLE   
DESCRIPTION
E 
PR 
C 
P 
Young’s modulus. 
Poisson’s ratio. 
Strain rate parameter, 𝐶, (Cowper Symonds). 
Strain rate parameter, 𝑃, (Cowper Symonds). 
LCSS 
Curve ID or Table ID. 
1.  Case  1:  LCSS  is  a  curve  ID.    The  curve  defines  effective 
stress as a function of total effective strain. 
2.  Case  2:  LCSS  is  a  table  ID.    Each  strain  rate  value  in  the 
table  is  associated  to  a  curve  ID  giving  the  stress  as  a 
function of effective strain for that rate. 
The  strain  rate  values  defined  in  the  table  may  be  given
as  the  natural  logarithm  of  the  strain  rate.    If  the  first
stress-strain  curve  in  the  table  corresponds  to  a  negative 
strain rate, LS-DYNA assumes that the natural logarithm 
of the strain rate value is used.  Since the tables are inter-
nally  discretized  to  equally  space  the  points,  natural
logarithms are necessary, for example, if the curves corre-
spond to rates from 10−4 to 104. 
LCSR 
Load curve ID defining strain rate scaling effect on yield stress.  If
LCSR  is  negative,  the  load  curve  is  evaluated  using  a  binary
search  for  the  correct  interval  for  the  strain  rate.    The  binary
search is slower than the default incremental search, but in cases
where  large  changes  in  the  strain  rate  may  occur  over  a  single
time step, it is more robust. 
EFTX 
Failure flag. 
EQ.0.0: failure determined by maximum tensile strain (default),
EQ.1.0: failure  determined  only  by  tensile  strain  in  local  𝑥
direction, 
EQ.2.0: failure  determined  only  by  tensile  strain  in  local  𝑦
direction. 
DAMP 
Stiffness-proportional damping  ratio.    Typical  values  are 10−3  or 
10−4.  If set too high instabilities can result.
Filtering  factor  for  strain  rate  effects.    Must  be  between  0  (no
filtering) and 1 (infinite filtering).  The filter is a simple low pass
filter  to  remove  high  frequency  oscillation  from  the  strain  rates
before  they  are  used  in  rate  effect  calculations.    The  cut  off 
frequency of the filter is [(1 - RFAC) / timestep] rad/sec. 
Load  curve  ID  giving  variation  of  failure  strain  with  strain  rate.
The points on the 𝑥-axis should be natural log of strain rate, the 𝑦-
axis  should  be  the  true  strain  to  failure.    Typically  this  is 
measured by uniaxial tensile test, and the strain values converted
to true strain. 
*MAT_089 
  VARIABLE   
RFAC 
LCFAIL 
Remarks: 
1.  M89  vs.    M24.    MAT_089  is  the  same  as  MAT_024  except  for  the  following 
points: 
•  Load  curve  lookup  for  yield  stress  is  based  on  equivalent  uniaxial  strain, 
not plastic strain (Remarks 2 and 3) 
•  elastic stiffness is initially equal to 𝐸 but will be increased according to the 
slope of the stress-strain curve (Remark 7) 
•  special strain calculation used for failure and damage (Remark 2) 
•  failure strain depends on strain rate (Remark 4) 
2.  Strain  Calculation  for  Failure  and  Damage.    The  strain  used  for  failure  and 
damage calculation, 𝜀pm is based on an approximation of the greatest value of 
maximum principal strain encountered during the analysis: 
𝜀pm = max
i≤n
where 
𝑛 = current time step index 
(𝜀𝐻
𝑖 + 𝜀VM
) 
max
𝑖≤𝑛
(. . . ) = maximum value attained by the argument during the calculation 
𝜀𝐻 =
𝜀𝑥 + 𝜀𝑦 + 𝜀𝑧
𝜀𝑥, 𝜀𝑦, 𝜀𝑧 = cumulative strain in the local x, y, or z direction 
𝜀vm = √
tr(𝛆′T𝛆′), the usual definition of equivalent uniaxial strain 
𝛆′ = deviatoric strain tensor, where each 𝜀𝑥, 𝜀𝑦, and 𝜀𝑧 is cumulative
3.  Yield Stress Load Curves.  When looking up yield stress from the load curve 
LCSS, the 𝑥-axis value is 𝜀vm. 
4.  Failure Strain Load Curves. 
𝜀sr =
d𝜀pm
d𝑡
= strain rate for failure and damage calculation 
𝜀𝐹 = LCFAIL(𝜀𝑠𝑟) 
= Instantanous true strain to failure from look-up on the curve LCFAIL 
5.  Damage.  A damage approach is used to avoid sudden shocks when the failure 
strain is reached.  Damage begins when the "strain ratio," 𝑅, reaches 1.0, where 
𝑅 = ∫
𝑑𝜀pm
𝜀𝐹
. 
Damage  is  complete,  and  the  element  fails  and  is  deleted,  when  𝑅 = 1.1.    The 
damage, 
𝐷 =
{⎧1.0
⎩{⎨
10(1.1 − 𝑅) 1.0 < 𝑅 < 1.1
 𝑅 < 1.0
is  a  reduction  factor  applied  to  all  stresses,  for  example,  when  𝑅  = 1.05,  then 
𝐷 = 0.5. 
6.  Strain  Definitions.    Unlike  other  LS-DYNA  material  models,  both  the  input 
stress-strain  curve  and  the  strain  to  failure  are  defined  as  total true  strain,  not 
plastic  strain.    The  input  can  be  defined  from  uniaxial  tensile  tests;  nominal 
stress  and  nominal  strain  from  the  tests  must  be  converted  to  true  stress  and 
true strain.  The elastic component of strain must not be subtracted out. 
7.  Elastic Stiffness Scaling.  The stress-strain curve is permitted to have sections 
steeper (i.e.  stiffer) than the elastic modulus.  When these are encountered the 
elastic modulus is increased to prevent spurious energy generation.  The elastic 
stiffness is scaled by a factor 𝑓e, which is calculated as follows: 
𝑓𝑒 = max (1.0,
𝑠max
3𝐺
) 
where 
𝐺 = initial shear modulus 
𝑆max = maximum slope of stress-strain curve encountered during the analysis 
8.  Precision.  Double precision is recommended when using this material model, 
especially if the strains become high. 
9.  Shell Numbering.  Invariant shell numbering is recommended when using this 
material model.  See *CONTROL_ACCURACY.
*MAT_ACOUSTIC 
This  is  Material  Type  90.    This  model  is  appropriate  for  tracking  low  pressure  stress 
waves in an acoustic media such as air or water and can be used only with the acoustic 
pressure  element  formulation.    The  acoustic  pressure  element  requires  only  one 
unknown  per  node.    This  element  is  very  cost  effective.    Optionally,  cavitation  can  be 
allowed. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
  Card 2 
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
3 
C 
F 
3 
ZP 
F 
4 
BETA 
F 
4 
XN 
F 
5 
CF 
F 
5 
YN 
F 
6 
7 
8 
ATMOS 
GRAV 
F 
7 
8 
F 
6 
ZN 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
C 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Sound speed 
BETA 
Damping factor.  Recommend values are between 0.1 and 1.0. 
CF 
Cavitation flag: 
EQ.0.0: off, 
EQ.1.0: on. 
ATMOS 
Atmospheric pressure (optional) 
GRAV 
Gravitational acceleration constant (optional) 
XP 
YP 
2-484 (EOS) 
x-coordinate of free surface point
VARIABLE   
DESCRIPTION
ZP 
XN 
YN 
ZN 
z-coordinate of free surface point 
x-direction cosine of free surface normal vector 
y-direction cosine of free surface normal vector 
z-direction cosine of free surface normal vector
*MAT_091-092 
*MAT_SOFT_TISSUE_{OPTION} 
Available options include: 
<BLANK> 
VISCO  
*MAT_SOFT_TISSUE 
This is Material Type 91 (OPTION=<BLANK>) or Material Type 92 (OPTION = VISCO).  
This  material  is  a  transversely  isotropic  hyperelastic  model  for  representing  biological 
soft  tissues  such  as  ligaments,  tendons,  and  fascia.    The  representation  provides  an 
isotropic Mooney-Rivlin matrix reinforced by fibers having a strain energy contribution 
with  the  qualitative  material  behavior  of  collagen.    The  model  has  a  viscoelasticity 
option which activates a six-term Prony series kernel for the relaxation function.  In this 
case,  the  hyperelastic  strain  energy  represents  the  elastic  (long-time)  response.    See 
Weiss et al.  [1996] and Puso and Weiss [1998] for additional details. 
NOTE: This material does not support specification of a ma-
terial  angle,  𝛽𝑖,  for  each  through-thickness  integra-
tion point of a shell. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
Variable 
1 
XK 
2 
RO 
F 
2 
3 
C1 
F 
3 
4 
C2 
F 
4 
5 
C3 
F 
5 
6 
C4 
F 
6 
7 
C5 
F 
7 
XLAM 
FANG 
XLAM0 
FAILSF 
FAILSM 
FAILSHR 
Type 
F 
F 
F 
F 
F 
F 
F 
  Card 3 
1 
Variable 
AOPT 
Type 
F 
2 
AX 
F 
3 
AY 
F 
4 
AZ 
F 
5 
BX 
F 
6 
BY 
F 
7 
BZ 
F 
8 
8
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LA1 
LA2 
LA3 
MACF 
Type 
F 
F 
F 
I 
Prony Series Card 1.  Additional card for VISCO keyword option.  
  Card 5 
Variable 
1 
S1 
Type 
F 
2 
S2 
F 
3 
S3 
F 
4 
S4 
F 
5 
S5 
F 
6 
S6 
F 
Prony Series Card 2.  Additional card for VISCO keyword option. 
  Card 6 
Variable 
1 
T1 
Type 
F 
2 
T2 
F 
3 
T3 
F 
4 
T4 
F 
5 
T5 
F 
6 
T6 
F 
7 
8 
7 
8 
  VARIABLE   
MID 
DESCRIPTION
Material  identification. 
exceeding 8 characters must be specified. 
  A  unique  number  or  label  not
RO 
Mass density 
C1 - C5 
Hyperelastic coefficients  
XK 
Bulk Modulus 
XLAM 
FANG 
Stretch ratio at which fibers are straightened 
Fiber angle in local shell coordinate system (shells only) 
XLAM0 
Initial fiber stretch (optional) 
FAILSF 
Stretch  ratio  for  ligament  fibers  at  failure  (applies  to  shell
elements only).  If zero, failure is not considered.
VARIABLE   
FAILSM 
FAILSHR 
DESCRIPTION
Stretch ratio for surrounding matrix material at failure (applies 
to shell elements only).  If zero, failure is not considered. 
Shear  strain  at  failure  at  a  material  point  (applies  to  shell 
elements only).  If zero, failure is not considered.  This failure
value is independent of FAILSF and FAILSM. 
AOPT 
Material axes option, see Figure M2-1 (bricks only): 
EQ.0.0: locally orthotropic with material axes determined by
element nodes as shown in Figure M2-1.  Nodes 1, 2, 
and  4  of  an  element  are  identical  to  the  nodes  used 
for the definition of a  coordinate system as  by *DE-
FINE_COORDINATE_NODES. 
EQ.1.0: locally orthotropic with material axes determined by
a  point  in  space  and  the  global  location  of  the  ele-
ment center; this is the 𝑎-direction.  This option is for 
solid elements only. 
EQ.2.0: globally  orthotropic  with  material  axes  determined
by vectors defined below, as with *DEFINE_COOR-
DINATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by  a
line in the plane of the element defined by the cross
product  of  the  vector  𝐯  with  the  element  normal. 
The  plane  of  a  solid  element  is  the  midsurface  be-
tween the inner surface and outer surface defined by
the  first  four  nodes  and  the  last  four  nodes  of  the
connectivity of the element, respectively. 
EQ.4.0: locally  orthotropic  in  cylindrical  coordinate  system
with the material axes determined by a vector 𝐯, and 
an  originating  point,  𝐩,  which  define  the  centerline 
axis.  This option is for solid elements only. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system
ID  number  (CID  on  *DEFINE_COORDINATE_-
or 
NODES, 
*DEFINE_COORDINATE_VECTOR).    Available  in 
R3 version of 971 and later. 
*DEFINE_COORDINATE_SYSTEM 
AX, AY, AZ 
Equal to XP, YP, ZP for AOPT = 1, 
Equal to A1, A2, A3 for AOPT = 2, 
Equal to V1, V2, V3 for AOPT = 3 or 4.
VARIABLE   
BX, BY, BZ 
DESCRIPTION
Equal to D1, D2, D3 for AOPT = 2 
Equal to XP, YP, ZP for AOPT = 4 
LAX, LAY, LAZ 
Local fiber orientation vector (bricks only) 
MACF 
Material axes change flag for brick elements: 
EQ.1: No change, default, 
EQ.2: switch material axes 𝑎 and 𝑏, 
EQ.3: switch material axes 𝑎 and 𝑐, 
EQ.4: switch material axes 𝑏 and 𝑐. 
Factors in the Prony series. 
Characteristic  times  for  Prony  series  relaxation  kernel  for
VISCO option. 
S1 – S6 
T1 - T6 
Remarks: 
The overall strain energy 𝑊 is "uncoupled" and includes two isotropic deviatoric matrix 
terms, a fiber term 𝐹, and a bulk term: 
𝑊 = 𝐶1(𝐼 ̃1 − 3) + 𝐶2(𝐼 ̃2 − 3) + 𝐹(𝜆) +
𝐾[ln(𝐽)]2 
Here, 𝐼 ̃1 and 𝐼 ̃2 are the deviatoric invariants of the right Cauchy deformation tensor, 𝜆 is 
the  deviatoric  part  of  the  stretch  along  the  current  fiber  direction,  and  𝐽 = det𝐅  is  the 
volume  ratio.    The  material  coefficients  𝐶1  and  𝐶2  are  the  Mooney-Rivlin  coefficients, 
while K is the effective bulk modulus of the material (input parameter XK). 
The  derivatives  of  the  fiber  term  𝐹  are  defined  to  capture  the  behavior  of  crimped 
collagen.  The fibers are assumed to be unable to resist compressive loading - thus the 
model is isotropic when 𝜆 < 1.  An exponential function describes the straightening of 
the  fibers,  while  a  linear  function  describes  the  behavior  of  the  fibers  once  they  are 
straightened past a critical fiber stretch level 𝜆 ≥ 𝜆∗ (input parameter XLAM): 
∂𝐹
∂𝜆
=
⎧
{{{{
{{{{
⎨
⎩
𝐶3
𝜆 < 1
[exp(𝐶4(𝜆 − 1)) − 1] 𝜆 < 𝜆∗
(𝐶5𝜆 + 𝐶6)
𝜆 ≥ 𝜆∗
Coefficients 𝐶3, 𝐶4, and 𝐶5 must be defined by the user.  𝐶6 is determined by LS-DYNA 
to ensure stress continuity at 𝜆 = 𝜆∗.  Sample values for the material coefficients 𝐶1 − 𝐶5
and 𝜆∗ for ligament tissue can be found in Quapp and Weiss [1998].  The bulk modulus 
𝐾 should be at least 3 orders of magnitude larger than 𝐶1 to ensure near-incompressible 
material behavior. 
Viscoelasticity  is  included  via  a  convolution  integral  representation  for  the  time-
dependent second Piola-Kirchoff stress 𝐒(𝐂, 𝑡): 
𝐒(𝐂, 𝑡) = 𝐒𝑒(𝐂) + ∫ 2𝐺(𝑡 − 𝑠)
𝜕𝑊
𝜕𝐂(𝑠)
𝑑𝑠
Here, 𝐒𝑒 is the elastic part of the second PK stress as derived from the strain energy, and 
𝐺(𝑡 − 𝑠) is the reduced relaxation function, represented by a Prony series: 
𝐺(𝑡) = ∑ 𝑆𝑖exp (
𝑖=1
𝑇𝑖
)
Puso and Weiss [1998] describe a graphical method to fit the Prony series coefficients to 
relaxation  data  that  approximates  the  behavior  of  the  continuous  relaxation  function 
proposed by Y-C.  Fung, as quasilinear viscoelasticity. 
Remarks on Input Parameters: 
Cards  1  through  4  must  be  included  for  both  shell  and  brick  elements,  although  for 
shells cards 3 and 4 are ignored and may be blank lines. 
For shell elements, the fiber direction lies in the plane of the element.  The local axis is 
defined by a vector between nodes n1 and n2, and the fiber direction may be offset from 
this axis by an angle FANG. 
For  brick  elements,  the  local  coordinate  system  is  defined  using  the  convention 
described  previously  for  *MAT_ORTHOTROPIC_ELASTIC.    The  fiber  direction  is 
oriented  in the  local  system  using  input  parameters  LAX,  LAY,  and  LAZ.    By  default, 
(LAX, LAY, LAZ) = (1,0,0) and the fiber is aligned with the local x-direction. 
An  optional  initial  fiber  stretch  can  be  specified  using  XLAM0.    The  initial  stretch  is 
applied  during  the  first  time  step.    This  creates  preload  in  the  model  as  soft  tissue 
contacts  and  equilibrium  is  established.    For  example,  a  ligament  tissue  "uncrimping 
strain" of 3% can be represented with initial stretch value of 1.03. 
If the VISCO option is selected, at least one Prony series term (S1, T1) must be defined.
*MAT_ELASTIC_6DOF_SPRING_DISCRETE_BEAM 
This  is  Material  Type  93.    This  material  model  is  defined  for  simulating  the  effects  of 
nonlinear  elastic  and  nonlinear  viscous  beams  by  using  six  springs  each  acting  about 
one  of  the  six  local  degrees-of-freedom.    The  input  consists  of  part  ID's  that  reference 
material  type,  *MAT_ELASTIC_SPRING_DISCRETE_BEAM  above  (type  74  above).  
Generally, these referenced parts are used only for the definition of this material model 
and  are  not  referenced  by  any  elements.    The  two  nodes  defining  a  beam  may  be 
coincident to give a zero length beam, or offset to give a finite length beam.  For finite 
length  discrete  beams  the  absolute  value  of  the  variable  SCOOR  in  the  SECTION_-
BEAM input should be set to a value of 2.0, which causes the local r-axis to be aligned 
along  the  two  nodes  of  the  beam  to  give  physically  correct  behavior.    The  distance 
between the nodes of a beam should not affect the behavior of this material model.  A 
triad is used to orient the beam for the directional springs. 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
4 
5 
6 
7 
8 
TPIDR 
TPIDS 
TPIDT 
RPIDR 
RPIDS 
RPIDT 
Type 
A8 
F 
I 
I 
I 
I 
I 
I 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density, see also volume in *SECTION_BEAM definition. 
TPIDR 
TPIDS 
TPIDT 
RPIDR 
RPIDS 
Translational  motion  in  the  local  r-direction  is  governed  by  part 
ID TPIDR.  If zero, no force is computed in this direction. 
Translational  motion  in  the  local  s-direction  is  governed  by  part 
ID TPIDS.  If zero, no force is computed in this direction. 
Translational  motion  in  the  local  t-direction  is  governed  by  part 
ID TPIDT.  If zero, no force is computed in this direction. 
Rotational  motion  about  the  local  r-axis  is  governed  by  part  ID 
RPIDR.  If zero, no moment is computed about this axis. 
Rotational  motion  about  the  local  s-axis  is  governed  by  part  ID 
RPIDS.  If zero, no moment is computed about this axis.
RPIDT 
*MAT_ELASTIC_6DOF_SPRING_DISCRETE_BEAM 
DESCRIPTION
Rotational  motion  about  the  local  t-axis  is  governed  by  part  ID 
RPIDT.  If zero, no moment is computed about this axis.
*MAT_INELASTIC_SPRING_DISCRETE_BEAM 
This is Material Type 94.  This model permits elastoplastic springs with damping to be 
represented with a discrete beam element type 6.  A yield force versus deflection curve 
is used which can vary in tension and compression. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
Variable 
FLCID 
HLCID 
Type 
F 
F 
3 
K 
F 
3 
C1 
F 
4 
F0 
F 
4 
C2 
F 
5 
D 
F 
5 
6 
7 
8 
CDF 
TDF 
F 
6 
F 
7 
8 
DLE 
GLCID 
F 
I 
  VARIABLE   
DESCRIPTION
MID 
RO 
K 
F0 
D 
CDF 
TDF 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density, see also volume in *SECTION_BEAM definition. 
Elastic loading/unloading stiffness.  This is required input. 
Optional  initial  force.    This  option  is  inactive  if  this  material  is
referenced in a part referenced by material type *MAT_INELAS-
TIC_6DOF_SPRING 
Optional viscous damping coefficient. 
Compressive displacement at failure.  Input as a positive number.
After failure, no forces are carried.  This option does not apply to
zero length springs. 
EQ.0.0: inactive. 
Tensile  displacement  at  failure.    After  failure,  no  forces  are
carried. 
EQ.0.0: inactive.
FLCID 
*MAT_INELASTIC_SPRING_DISCRETE_BEAM 
DESCRIPTION
Load  curve  ID,  see  *DEFINE_CURVE,  defining  the  yield  force 
versus  plastic  deflection.    If  the  origin  of  the  curve  is  at  (0,0)  the
force magnitude is identical in tension and compression, i.e., only
the  sign  changes.    If  not,  the  yield  stress  in  the  compression  is 
used when the spring force is negative.  The plastic displacement
increases  monotonically  in  this  implementation.    The  load  curve
is required input. 
HLCID 
Load  curve  ID,  see  *DEFINE_CURVE,  defining  force  versus 
relative velocity (Optional).  If the origin of the curve is at (0,0) the
force magnitude is identical for a given magnitude of the relative
velocity, i.e., only the sign changes. 
C1 
C2 
Damping coefficient. 
Damping coefficient 
DLE 
Factor to scale time units. 
GLCID 
Optional  load  curve  ID,  see  *DEFINE_CURVE,  defining  a  scale 
factor versus deflection for load curve ID, HLCID.  If zero, a scale
factor of unity is assumed. 
Remarks: 
The yield force is taken from the load curve: 
𝐹𝑌 = 𝐹𝑦(Δ𝐿plastic) 
where 𝐿plastic is the plastic deflection.  A trial force is computed as: 
and is checked against the yield force to determine 𝐹: 
𝐹𝑇 = 𝐹𝑛 + K × Δ𝐿̇(Δ𝑡) 
𝐹 = {
𝐹𝑌  𝑖𝑓   𝐹𝑇 > 𝐹𝑌
𝐹𝑇  𝑖𝑓   𝐹𝑇 ≤ 𝐹𝑌 
The final force, which includes rate effects and damping, is given by: 
𝐹𝑛+1 = 𝐹 × [1 + C1 × Δ𝐿̇ + C2 × sgn(Δ𝐿̇)ln (max {1. ,
∣Δ𝐿̇∣
DLE
})] + D×Δ𝐿̇ + 𝑔(Δ𝐿)ℎ(Δ𝐿̇) 
Unless the origin of the curve starts at (0,0), the negative part of the curve is used when 
the  spring  force  is  negative  where  the  negative  of  the  plastic  displacement  is  used  to 
interpolate, 𝐹𝑦.  The positive part of the curve is used whenever the force is positive.  In 
these equations, Δ𝐿 is the change in length
Δ𝐿 = current  length - initial  length 
The  cross  sectional  area  is  defined  on  the  section  card  for  the  discrete  beam  elements, 
See  *SECTION_BEAM.    The  square  root  of  this  area  is  used  as  the  contact  thickness 
offset if these elements are included in the contact treatment.
*MAT_INELASTIC_6DOF_SPRING_DISCRETE_BEAM 
type,  *MAT_INELASTIC_SPRING_DISCRETE_BEAM  above 
This  is  Material  Type  95.    This  material  model  is  defined  for  simulating  the  effects  of 
nonlinear inelastic and nonlinear viscous beams by using six springs each acting about 
one  of  the  six  local  degrees-of-freedom.    The  input  consists  of  part  ID's  that  reference 
material 
(type  94).  
Generally, these referenced parts are used only for the definition of this material model 
and  are  not  referenced  by  any  elements.    The  two  nodes  defining  a  beam  may  be 
coincident to give a zero length beam, or offset to give a finite length beam.  For finite 
length  discrete  beams  the  absolute  value  of  the  variable  SCOOR  in  the  SECTION_-
BEAM input should be set to a value of 2.0, which causes the local r-axis to be aligned 
along  the  two  nodes  of  the  beam  to  give  physically  correct  behavior.    The  distance 
between the nodes of a beam should not affect the behavior of this material model.  A 
triad must be used to orient the beam for zero length beams. 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
4 
5 
6 
7 
8 
TPIDR 
TPIDS 
TPIDT 
RPIDR 
RPIDS 
RPIDT 
Type 
A8 
F 
I 
I 
I 
I 
I 
I 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density, see also volume in *SECTION_BEAM definition. 
TPIDR 
TPIDS 
TPIDT 
RPIDR 
RPIDS 
Translational  motion  in  the  local  r-direction  is  governed  by  part 
ID TPIDR. If zero, no force is computed in this direction. 
Translational  motion  in  the  local  s-direction  is  governed  by  part 
ID TPIDS. If zero, no force is computed in this direction. 
Translational  motion  in  the  local  t-direction  is  governed  by  part 
ID TPIDT. If zero, no force is computed in this direction. 
Rotational  motion  about  the  local  r-axis  is  governed  by  part  ID 
RPIDR.  If zero, no moment is computed about this axis. 
Rotational  motion  about  the  local  s-axis  is  governed  by  part  ID 
RPIDS.  If zero, no moment is computed about this axis.
VARIABLE   
RPIDT 
DESCRIPTION
Rotational  motion  about  the  local  t-axis  is  governed  by  part  ID 
RPIDT.  If zero, no moment is computed about this axis.
This is Material Type 96. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
*MAT_BRITTLE_DAMAGE 
3 
E 
F 
3 
4 
PR 
F 
4 
5 
6 
7 
8 
TLIMIT 
SLIMIT 
FTOUGH 
SRETEN 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
VISC 
FRA_RF 
E_RF 
YS_RF 
EH_RF 
FS_RF 
SIGY 
Type 
F 
F 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young's modulus. 
Poisson's ratio. 
TLIMIT 
Tensile limit. 
SLIMIT 
Shear limit. 
FTOUGH 
Fracture toughness. 
SRETEN 
Shear retention. 
VISC 
Viscosity. 
FRA_RF 
Fraction of reinforcement in section. 
E_RF 
Young's modulus of reinforcement. 
YS_RF 
Yield stress of reinforcement. 
EH_RF 
Hardening modulus of reinforcement.
VARIABLE   
DESCRIPTION
Failure strain (true) of reinforcement. 
Compressive yield stress. 
EQ.0: no compressive yield 
FS_RF 
SIGY 
Remarks: 
A full description of the tensile and shear damage parts of this material model is given 
in  Govindjee,  Kay  and  Simo  [1994,1995].    It  is  an  anisotropic  brittle  damage  model 
designed  primarily  for  concrete  though  it  can  be  applied  to  a  wide  variety  of  brittle 
materials.    It  admits  progressive  degradation  of  tensile  and  shear  strengths  across 
smeared  cracks  that  are  initiated  under  tensile  loadings.    Compressive  failure  is 
governed by a simplistic J2 flow correction that can be disabled if not desired.  Damage 
is handled by treating the rank 4 elastic stiffness tensor as an evolving internal variable 
for the material.  Softening induced mesh dependencies are handled by a characteristic 
length method [Oliver 1989]. 
Description of properties: 
1.  E is the Young's modulus of the undamaged material also known as the virgin 
modulus. 
2.  υ  is  the  Poisson's  ratio  of  the  undamaged  material  also  known  as  the  virgin 
Poisson's ratio. 
3. 
𝑓𝑛 is the initial principal tensile strength (stress) of the material.  Once this stress 
has been reached at a point in the body a smeared crack is initiated there with a 
normal  that  is  co-linear  with  the  1st  principal  direction.    Once  initiated,  the 
crack  is  fixed  at  that  location,  though  it  will  convect  with  the  motion  of  the 
body.    As  the  loading  progresses  the  allowed  tensile  traction  normal  to  the 
crack plane is progressively degraded to a small machine dependent constant.  
The degradation is implemented by reducing the material's modulus normal to 
the smeared crack plane according to a maximum dissipation law that incorpo-
rates exponential softening.  The restriction on the normal tractions is given by 
𝜙𝑡 = (𝐧 ⊗ 𝐧): σ − 𝑓𝑛 + (1 − 𝜀)𝑓𝑛(1 − exp[−𝐻𝛼]) ≤ 0 
where 𝐧 is the smeared crack normal, 𝜀 is the small constant, 𝐻 is the softening 
modulus, and 𝛼 is an internal variable.  𝐻 is set automatically by the program; 
see 𝑔𝑐 below.  𝛼 measures the crack field intensity and is output in the equiva-
lent plastic strain field, 𝜀̅𝑝, in a normalized fashion.
The  evolution  of  alpha  is  governed  by  a  maximum  dissipation  argument.  
When the normalized value reaches unity it means that the material's strength 
has  been  reduced  to  2%  of  its  original  value  in  the  normal  and  parallel  direc-
tions  to  the  smeared  crack.    Note  that  for  plotting  purposes  it  is  never  output 
greater than 5. 
4. 
𝑓𝑠  is  the  initial  shear  traction  that  may  be  transmitted  across  a  smeared  crack 
plane.    The  shear  traction  is  limited  to  be  less  than  or  equal  to  𝑓𝑠(1 − 𝛽)(1 −
exp[−𝐻𝛼]),  through  the  use  of  two  orthogonal  shear  damage  surfaces.    Note 
that  the  shear  degradation  is  coupled  to  the  tensile  degradation  through  the 
internal variable alpha which measures the intensity of the crack field. 𝛽 is the 
shear retention factor defined below.  The shear degradation is taken care of by 
reducing the material's shear stiffness parallel to the smeared crack plane. 
5. 
𝑔𝑐  is  the  fracture  toughness  of  the  material.    It  should  be  entered  as  fracture 
energy  per  unit  area  crack  advance.    Once  entered  the  softening  modulus  is 
automatically calculated based on element and crack geometries.  
6.  𝛽  is  the  shear  retention  factor.    As  the  damage  progresses  the  shear  tractions 
allowed across the smeared crack plane asymptote to the product 𝛽𝑓𝑠. 
7.  𝜂 represents the viscosity of the material.  Viscous behavior is implemented as a 
simple  Perzyna  regularization  method.    This  allows  for  the  inclusion  of  first 
order rate effects.  The use of some viscosity is recommend as it serves as regu-
larizing parameter that increases the stability of calculations. 
8.  𝜎𝑦  is  a  uniaxial  compressive  yield  stress.    A  check  on  compressive  stresses  is 
made using the J2 yield function 𝐬: 𝐬 − √2
3 𝜎𝑦 ≤ 0, where 𝐬 is the stress deviator.  
If violated, a J2 return mapping correction is executed.  This check is executed 
when (1) no damage has taken place at an integration point yet,  (2) when dam-
age has taken place at a point but the crack is currently closed, and (3) during 
active damage after the damage integration (i.e.  as an operator split).  Note that 
if the crack is open the plasticity correction is done in the plane-stress subspace 
of the crack plane. 
A variety of experimental data has been replicated using this model from quasi-static to 
explosive  situations.    Reasonable  properties  for  a  standard  grade  concrete  would  be 
E = 3.15x106  psi,  𝑓𝑛 = 450  psi,  𝑓𝑠 = 2100  psi,  𝜈 = 0.2,  𝑔𝑐 = 0.8  lbs/in,  𝛽 = 0.03,  𝜂 = 0.0  psi-
sec, 𝜎𝑦 = 4200 psi.  For stability, values of 𝜂 between 104 to 106 psi/sec are recommend-
ed.    Our  limited  experience  thus  far  has  shown  that  many  problems  require  nonzero 
values of 𝜂 to run to avoid error terminations. 
Various  other  internal  variables  such  as  crack  orientations  and  degraded  stiffness 
tensors are internally calculated but currently not available for output.
*MAT_GENERAL_JOINT_DISCRETE_BEAM 
This is Material Type 97.  This model is used to define a general joint constraining any 
combination of degrees of freedom between two nodes.  The nodes may belong to rigid 
or  deformable  bodies.    In  most  applications  the  end  nodes  of  the  beam  are  coincident 
and the local coordinate system (r,s,t axes) is defined by CID . 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
TR 
I 
4 
TS 
I 
5 
TT 
I 
6 
RR 
I 
7 
RS 
I 
8 
RT 
Remarks 
1 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RPST 
RPSR 
Type 
Remarks 
F 
2 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
TR 
TS 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density, see also volume in *SECTION_BEAM definition. 
Translational  constraint  code  along  the  r-axis  (0 ⇒  free,  1 ⇒
constrained) 
Translational  constraint  code  along  the  s-axis  (0 ⇒  free,  1 ⇒
constrained)
*MAT_GENERAL_JOINT_DISCRETE_BEAM 
DESCRIPTION
TT 
RR 
RS 
RT 
RPST 
RPSR 
Remarks: 
Translational  constraint  code  along  the  t-axis  (0 ⇒  free,  1 ⇒ 
constrained) 
Rotational  constraint  code  about  the  r-axis  (0 ⇒  free,  1 ⇒
constrained) 
Rotational  constraint  code  about  the  s-axis  (0 ⇒  free,  1 ⇒
constrained) 
Rotational  constraint  code  about  the  t-axis  (0 ⇒  free,  1 ⇒
constrained) 
Penalty stiffness scale factor for translational constraints. 
Penalty stiffness scale factor for rotational constraints. 
1.  For  explicit  calculations,  the  additional  stiffness  due  to  this  joint  may  require 
addition  mass  and  inertia  for  stability.    Mass  and  rotary  inertia  for  this  beam 
element  is  based  on  the  defined  mass  density,  the  volume,  and  the  mass  mo-
ment of inertia defined in the *SECTION_BEAM input. 
2.  The  penalty  stiffness  applies  to  explicit  calculations.    For  implicit  calculations, 
constraint equations are generated and imposed on the system equations; there-
fore, these constants, RPST and RPSR, are not used.
*MAT_SIMPLIFIED_JOHNSON_COOK_{OPTION} 
Available options include: 
<BLANK> 
STOCHASTIC 
This  is  Material  Type  98  implementing  Johnson/Cook  strain  sensitive  plasticity.    It  is 
used for problems where the strain rates vary over a large range.  In contrast to the full 
Johnson/Cook  model  (material  type  15)  this  model 
introduces  the  following 
simplifications: 
1. 
2. 
thermal effects and damage are ignored, 
and  the  maximum  stress  is  directly  limited  since  thermal  softening  which  is 
very  significant  in  reducing  the  yield  stress  under  adiabatic  loading  is  not 
available. 
An  iterative  plane  stress  update  is  used  for  the  shell  elements,  but  due  to  the 
simplifications related to thermal softening and damage, this model is 50% faster than 
the  full  Johnson/Cook  implementation.    To  compensate  for  the  lack  of  thermal 
softening,  limiting  stress  values  are  introduced  to  keep  the  stresses  within  reasonable 
limits. 
A  resultant  formulation  for  the  Belytschko-Tsay,  the  C0  Triangle,  and  the  fully 
integrated type 16 shell elements is available and can be activated by specifying either 
zero or one through thickness integration point on the *SECTION_SHELL card.  While 
less accurate than through thickness integration, this formulation runs somewhat faster.  
Since the stresses are not computed in the resultant formulation, the stresses written to 
the databases for the resultant elements are set to zero. 
This model is also available for the Hughes-Liu beam, the Belytschko-Schwer beam, and 
for  the  truss  element.    For  the  resultant  beam  formulation,  the  rate  effects  are 
approximated by the axial rate, since the thickness of the beam about it bending axes is 
unknown.  Because this model is primarily used for structural analysis, the pressure is 
determined using the linear bulk modulus.
Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
VP 
F 
Default 
none 
none 
none 
none 
0.0 
6 
7 
8 
  Card 2 
Variable 
Type 
1 
A 
F 
2 
B 
F 
3 
N 
F 
4 
C 
F 
5 
6 
7 
8 
PSFAIL 
SIGMAX 
SIGSAT 
EPSO 
F 
F 
F 
F 
Default 
none 
0.0 
0.0 
0.0 
1.0E+17 SIGSAT  1.0E+28 
1.0 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
VP 
A 
B 
N 
C 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s modulus 
Poisson’s ratio 
Formulation for rate effects: 
EQ.0.0: Scale yield stress (default), 
EQ.1.0: Viscoplastic formulation. 
This option applies only to the 4-node shell and 8-node thick shell 
if and only if through thickness integration is used. 
See equations below. 
See equations below. 
See equations below. 
See equations below.
VARIABLE   
DESCRIPTION
PSFAIL 
Effective plastic strain at failure.  If zero failure is not considered. 
Maximum  stress  obtainable  from  work  hardening  before  rate
effects are added (optional).  This option is ignored if VP = 1.0 
Saturation  stress  which  limits  the  maximum  value  of  effective 
stress which can develop after rate effects are added (optional). 
Quasi-static threshold strain rate.  See description under *MAT_-
015. 
SIGMAX 
SIGSAT 
EPS0 
Remarks: 
Johnson and Cook express the flow stress as 
𝜎𝑦 = (𝐴 + 𝐵𝜀̅ 𝑝𝑛
)(1 + 𝐶 ln 𝜀∗̇ ) 
where 
𝐴, 𝐵, 𝐶  = input constants 
𝜀̅𝑝 = effective plastic strain 
𝜀∗̇ =
𝜀̅
EPS0
= normalized effective strain rate 
The maximum stress is limited by SIGMAX and SIGSAT by: 
𝜎𝑦 = min{min[𝐴 + 𝐵𝜀̅ 𝑝𝑛
, SIGMAX](1 + 𝑐 ln 𝜀∗̇ ), SIGSAT} 
Failure occurs when the effective plastic strain exceeds PSFAIL. 
If  the  viscoplastic  option  is  active,  VP = 1.0,  the  parameters  SIGMAX  and  SIGSAT  are 
ignored  since  these  parameters  make  convergence  of  the  viscoplastic  strain  iteration 
loop  difficult  to  achieve.    The  viscoplastic  option  replaces  the  plastic  strain  in  the 
forgoing equations by the viscoplastic strain and the strain rate by the viscoplastic strain 
rate.  Numerical noise is substantially reduced by the viscoplastic formulation. 
The STOCHASTIC option allows spatially varying yield and failure behavior.  See *DE-
FINE_STOCHASTIC_VARIATION for additional information.
LS-DYNA R10.0
*MAT_SIMPLIFIED_JOHNSON_COOK_ORTHOTROPIC_DAMAGE 
This  is  Material  Type  99.    This  model,  which  is  implemented  with  multiple  through 
thickness integration points, is an extension of model 98 to include orthotropic damage 
as  a  means  of  treating  failure  in  aluminum  panels.    Directional  damage  begins  after  a 
defined  failure  strain  is  reached  in  tension  and  continues  to  evolve  until  a  tensile 
rupture strain is reached in either one of the two orthogonal directions.  After rupture is 
detected at NUMINT integration points, the element is deleted. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
VP 
F 
6 
7 
8 
EPPFR 
LCDM 
NUMINT 
F 
I 
I 
Default 
none 
none 
none 
none 
0.0 
1.e+16  optional 
all 
points 
  Card 2 
Variable 
Type 
1 
A 
F 
2 
B 
F 
3 
N 
F 
4 
C 
F 
5 
6 
7 
8 
PSFAIL 
SIGMAX 
SIGSAT 
EPSO 
F 
F 
F 
F 
Default 
none 
0.0 
0.0 
0.0 
1.0E+17 SIGSAT  1.0E+28 
1.0 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s modulus 
Poisson’s ratio
*MAT_SIMPLIFIED_JOHNSON_COOK_ORTHOTROPIC_DAMAGE  *MAT_099 
  VARIABLE   
DESCRIPTION
VP 
Formulation for rate effects: 
EQ.0.0: Scale yield stress (default), 
EQ.1.0: Viscoplastic formulation. 
EPPFR 
LCDM 
NUMINT 
This option applies only to the 4-node shell and 8-node thick shell 
if and only if through thickness integration is used. 
Plastic strain at which material ruptures (logarithmic). 
Load  curve  ID  defining  nonlinear  damage  curve.    See  Figure 
M81-2. 
Number  of  through  thickness  integration  points  which  must  fail
before the element is deleted.  (If zero, all points must fail.)  The
default  of  all  integration  points  is  not  recommended  since
elements  undergoing  large  strain  are  often  not  deleted  due  to
nodal  fiber  rotations  which  limit  0strains  at  active  integration
points after most points have failed.  Better results are obtained if
NUMINT is set to 1 or a number less than one half of the number
of  through  thickness  points.    For  example,  if  four  through
thickness points are used, NUMINT should not exceed 2, even for
fully integrated shells which have 16 integration points. 
A 
B 
N 
C 
See equations below. 
See equations below. 
See equations below. 
See equations below. 
PSFAIL 
Principal plastic strain at failure.  If zero failure is not considered.
SIGMAX 
SIGSAT 
EPS0 
Maximum  stress  obtainable  from  work  hardening  before  rate
effects are added (optional).  This option is ignored if VP = 1.0 
Saturation  stress  which  limits  the  maximum  value  of  effective
stress which can develop after rate effects are added (optional). 
Quasi-static threshold strain rate.  See description under *MAT_-
015.
*MAT_SIMPLIFIED_JOHNSON_COOK_ORTHOTROPIC_DAMAGE 
See the description for the SIMPLIFIED_JOHNSON_COOK model above.
*MAT_100 
This is Material Type 100.  The material model applies to beam element type 9 and to 
solid element type 1.  The failure models apply to both beam and solid elements. 
In the case of solid elements, if hourglass type 4 is specified then hourglass type 4 will 
be used, otherwise, hourglass type 6 will be automatically assigned.  Hourglass type 6 is 
preferred. 
The  beam  elements,  based  on  the  Hughes-Liu  beam  formulation,  may  be  placed 
between  any  two  deformable  shell  surfaces  and  tied  with  constraint  contact,  *CON-
TACT_SPOTWELD,  which  eliminates  the  need  to  have  adjacent  nodes  at  spot  weld 
locations.  Beam spot welds may be placed between rigid bodies and rigid/deformable 
bodies by making the node on one end of the spot weld a rigid body node which can be 
an extra node for the rigid body, see *CONSTRAINED_EXTRA_NODES_OPTION.   In 
the same way rigid bodies may also be tied  together with this spot weld option.  This 
weld  option  should  not  be  used  with  rigid  body  switching.    The  foregoing  advice  is 
valid if solid element spot welds are used; however, since the solid elements have just 
three  degrees-of-freedom  at  each  node,  *CONTACT_TIED_SURFACE_TO_SURFACE 
must be used instead of *CONTACT_SPOTWELD. 
In  flat  topologies the  shell  elements  have  an  unconstrained  drilling  degree-of-freedom 
which  prevents  torsional  forces  from  being  transmitted.    If  the  torsional  forces  are 
deemed to be important, brick elements should be used to model the spot welds. 
Beam  and  solid  element  force  resultants  for MAT_SPOTWELD  are  written  to the  spot 
weld  force  file,  swforc,  and  the  file  for  element  stresses  and  resultants  for  designated 
elements, elout. 
It  is  advisable  to  include  all  spot  welds,  which  provide  the  slave  nodes,  and  spot 
welded  materials,  which  define  the  master  segments,  within  a  single  *CONTACT_-
SPOTWELD  interface  for  beam  element  spot  welds  or  a  *CONTACT_TIED_SUR-
FACE_TO_SURFACE interface for solid element spot welds.  As a constraint method 
these interfaces are treated independently which can lead to significant problems if such 
interfaces share common nodal points.  An added benefit is that memory usage can be 
substantially less with a single interface. 
Available options include: 
<BLANK> 
DAMAGE-FAILURE 
The DAMAGE-FAILURE option causes one additional line to be read with the damage 
parameter and a flag that determines how failure is computed from the resultants.  On 
this  line  the  parameter,  RS,  if  nonzero,  invokes  damage  mechanics  combined  with  the 
plasticity model to achieve a smooth drop off of the resultant forces prior to the removal
of  the  spot  weld.    The  parameter  OPT  determines  the  method  used  in  computing 
resultant based failure, which is unrelated to damage. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
SIGY 
F 
6 
EH 
F 
7 
DT 
F 
Card 2 for no failure.  Additional card for <blank> keyword option. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
Variable 
EFAIL 
NRR 
NRS 
NRT 
MRR 
MSS 
MTT 
Type 
F 
F 
F 
F 
F 
F 
F 
8 
TFAIL 
F 
8 
NF 
F 
Card 2 for resultant based failure.  Additional card for DAMAGE-FAILURE keyword 
option with OPT = -1.0 or 0.0. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
Variable 
EFAIL 
NRR 
NRS 
NRT 
MRR 
MSS 
MTT 
Type 
F 
F 
F 
F 
F 
F 
F 
8 
NF 
F 
Card  2  for  stress  based  failure.    Additional  card  for  DAMAGE-FAILURE  keyword 
option with OPT = 1.0 and positive values in fields 2 and 3. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
Variable 
EFAIL 
SIGAX 
SIGTAU 
Type 
F 
F 
F 
8 
NF
Card  2  for  stress  based  failure.    Additional  card  for  DAMAGE-FAILURE  keyword 
option with OPT = 1.0 and negative values in fields 2 and 3. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
Variable 
EFAIL 
-LCAX 
-LCTAU 
Type 
F 
F 
F 
8 
NF 
F 
Card  2  for  user  subroutine  based  failure.    Additional  card  for DAMAGE-FAILURE 
keyword option with OPT = 2.0, 12, or 22. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
Variable 
EFAIL 
USRV1 
USRV2 
USRV3 
USRV4 
USRV5 
USRV6 
Type 
F 
F 
F 
F 
F 
F 
F 
Card 2 for OPT = 3.0 or 4.0. 
  Card 2 
1 
Variable 
EFAIL 
Type 
F 
Card 2 for OPT = 5.0. 
  Card 2 
1 
Variable 
EFAIL 
Type 
F 
2 
ZD 
F 
2 
ZD 
F 
3 
ZT 
F 
3 
ZT 
F 
4 
5 
6 
7 
ZALP1 
ZALP2 
ZALP3 
ZRRAD 
F 
F 
F 
F 
5 
6 
7 
8 
4 
ZT2 
F 
8 
NF 
F 
8 
NF
Card 2 for OPT = 6.0, 7.0, 9.0, or 10.0. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
Variable 
EFAIL 
Type 
F 
Card 2 for OPT = 11.0. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
Variable 
EFAIL 
LCT 
LCC 
Type 
F 
F 
F 
8 
NF 
F 
8 
NF 
F 
Additional card for the DAMAGE-FAILURE option.  
  Card 3 
Variable 
1 
RS 
2 
3 
4 
5 
6 
7 
8 
OPT 
FVAL 
TRUE_T 
ASFF 
BETA 
DMGOPT 
Type 
F 
F 
F 
F 
I 
F 
F 
Optional  2nd  additional  card  for  the  DAMAGE-FAILURE  option,  read  only  if 
DMGOPT = -1 on card 3. 
 Card 3A 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  DMGOPT 
FMODE 
FFCAP 
Type 
F 
F 
F 
Additional card for OPT = 12 or 22. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
USRV7 
USRV8 
USRV9 
USRV10 
USRV11 
USRV12 
USRV13 
USRV14 
Type 
F 
F 
F 
F 
F 
F 
F
Additional card for OPT = 12 or 22 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
USRV15 
USRV16 
USRV17 
USRV18 
USRV19 
USRV20 
USRV21 
USRV22 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
SIGY 
EH 
DT 
TFAIL 
EFAIL 
NRR 
NRS 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s modulus.  If input as negative, a uniaxial option for solid
spot welds is invoked; see “Uniaxial option” in remarks. 
Poisson’s ratio 
GT.0: Initial yield stress. 
LT.0:  A yield curve or table is assigned by |SIGY|. 
Plastic hardening modulus, 𝐸ℎ 
Time step size for mass scaling, Δ𝑡 
Failure time if nonzero.  If zero this option is ignored. 
Effective  plastic  strain  in  weld  material  at  failure.    If  the  damage
option  is  inactive,  the  spot  weld  element  is  deleted  when  the 
plastic  strain  at  each  integration  point  exceeds  EFAIL.    If  the
damage option is active, the plastic strain must exceed the rupture
strain (RS) at each integration point before deletion occurs. 
𝐹   at  failure 
Axial  force  resultant  𝑁𝑟𝑟𝐹  or  maximum  axial  stress  𝜎𝑟𝑟
depending on the value of OPT .  If zero, failure due to
this  component  is  not  considered.    If  negative,  |NRR|  is  the  load 
curve ID defining the maximum axial stress at failure as a function
of the effective strain rate. 
Force  resultant  𝑁𝑟𝑠𝐹  or  maximum  shear  stress  𝜏𝐹  at  failure 
depending on the value of OPT .  If zero, failure due to
this  component  is  not  considered.    If  negative,  |NRS|  is  the  load
VARIABLE   
DESCRIPTION
NRT 
MRR 
MSS 
MTT 
curve  ID  defining  the  maximum  shear  stress  at  failure  as  a
function of the effective strain rate. 
Force  resultant  𝑁𝑟𝑡𝐹  at  failure.    If  zero,  failure  due  to  this 
component is not considered. 
Torsional moment resultant 𝑀𝑟𝑟𝐹 at failure.  If zero, failure due to 
this component is not considered. 
Moment  resultant  𝑀𝑠𝑠𝐹  at  failure.    If  zero,  failure  due  to  this 
component is not considered. 
Moment  resultant  𝑀𝑡𝑡𝐹  at  failure.    If  zero,  failure  due  to  this 
component is not considered. 
NF 
Number of force vectors stored for filtering. 
SIGAX 
SIGTAU 
LCAX 
LCTAU 
Maximum  axial  stress  𝜎𝑟𝑟
component is not considered. 
𝐹   at  failure.    If  zero,  failure  due  to  this 
Maximum  shear  stress  𝜏𝐹  at  failure.    If  zero,  failure  due  to  this 
component is not considered. 
Load  curve  ID  defining  the  maximum  axial  stress  at  failure  as  a
function of the effective strain rate.  Input as a negative number. 
Load  curve  ID  defining  the  maximum  shear  stress  at  failure  as  a 
function of the effective strain rate.  Input as a negative number. 
USRVn 
Failure constants for user failure subroutine, 𝑛 = 1,2, … ,6 
ZD 
ZT 
Notch diameter 
Sheet thickness. 
ZALP1 
Correction factor alpha1 
ZALP2 
Correction factor alpha2 
ZALP3 
Correction factor alpha3 
ZRRAD 
Notch root radius (OPT = 3.0 only). 
ZT2 
LCT 
2-514 (EOS) 
Second sheet thickness (OPT = 5.0 only)
VARIABLE   
DESCRIPTION
LCC 
RS 
OPT 
under tension as a function of loading direction (in degree range 0
to 90).  Table defines these curves as functions of strain rates.  See
remarks.  (OPT = 11.0 only) 
Load curve or Table ID.  Load curve defines resultant failure force
under  compression  as  a  function  of  loading  direction  (in  degree
range  0  to  90).    Table  defines  these  curves  as  functions  of  strain
rates.  See remarks.  (OPT = 11.0 only) 
Rupture strain.  Define if and only if damage is active. 
Failure option: 
EQ.-9:  OPT = 9  failure  is  evaluated  and  written  to  the  swforc
file, but element failure is suppressed. 
EQ.-2:  same as option –1 but in addition, the peak value of the 
failure  criteria  and  the  time  it  occurs  is  stored  and  is
written into the swforc database.  This information may 
be  necessary  since  the  instantaneous  values  written  at
specified time intervals may miss the peaks.  Additional 
storage is allocated to store this information. 
EQ.-1:  OPT = 0 failure is evaluated and written into the swforc
file, but element failure is suppressed 
EQ.0:  resultant based failure 
EQ.1:  stress based failure computed from resultants (Toyota) 
EQ.2:  user subroutine uweldfail to determine failure 
EQ.3:  notch  stress  based  failure.    (beam  and  hex  assembly
welds only). 
EQ.4:  stress intensity factor at failure.  (beam and hex assembly
welds only). 
EQ.5:  structural stress at failure (beam and hex assembly welds 
only). 
EQ.6:  stress  based  failure  computed  from  resultants  (Toyota).
In this option a shell strain rate dependent failure model
is used (beam and hex assembly welds only).  The static
failure stresses are defined by part ID using the keyword 
*DEFINE_SPOTWELD_RUPTURE_STRESS. 
EQ.7:  stress based failure for solid elements (Toyota) with peak
stresses  computed  from  resultants,  and  strength  values
input  for  pairs  of  parts,  see  *DEFINE_SPOTWELD_-
VARIABLE   
DESCRIPTION
FAILURE_RESULTANTS.  Strain rate effects are option-
al. 
EQ.8:  not used. 
EQ.9:  stress  based  failure  from  resultants  (Toyota).    In  this
option a shell strain rate dependent failure model is used
(beam welds only).  The static failure stresses are defined
by  part  ID  using  the  keyword  *DEFINE_SPOTWELD_-
RUPTURE_PARAMETER. 
EQ.10:  stress  based  failure  with  rate  effects.    Failure  data  is
defined  by  material  using  the  keyword  *DEFINE_-
SPOWELD_FAILURE. 
EQ.11:  resultant based failure (beams only).  In this option load
curves  or  tables  LCT  (tension)  and  LCC  (compression) 
can  be  defined  as  resultant  failure  force  vs.    loading  di-
rection  (curve)  or  resultant  failure  force  vs.    loading  di-
rection vs.  strain rate (table). 
EQ.12:  user  subroutine  uweldfail12  with  22  material  constants
to determine damage and failure. 
EQ.22:  user  subroutine  uweldfail22  with  22  material  constants
to determine failure. 
FVAL 
Failure parameter.  If OPT: 
EQ.-2:  Not used. 
EQ.-1:  Not used. 
EQ.0:  Function 
ID 
(*DEFINE_FUNCTION) 
define 
alternative  Weld  Failure.    If  this  is  set,  the  values  given
for NRR, NRS, NRT, MRR, MSS and MTT in Card 2 are
ignored.   
to 
EQ.1:  Not used. 
EQ.2:  Not used. 
EQ.3:  Notch stress value at failure (KF). 
EQ.4:  Stress intensity factor value at failure (KeqF). 
EQ.5:  Structural stress value at failure (sF). 
EQ.6:  Number  of  cycles  that  failure  condition  must  be  met  to
trigger beam deletion. 
EQ.7:  Not used.
n5
n8
n4
n6
n7
n3
n1
n2
Figure M100-1.  A solid element used as spot weld is shown.  When resultant
based failure is used orientation is very important.  Nodes n1-n4 attach to the
lower shell mid-surface and nodes n5-n8 attach to the upper shell mid-surface.
The resultant forces and moments are computed based on the assumption that
the brick element is properly oriented. 
  VARIABLE   
DESCRIPTION
TRUE_T 
EQ.9:  Number  of  cycles  that  failure  condition  must  be  met  to 
trigger beam deletion. 
EQ.10:  ID of data defined by *DEFINE_SPOTWELD_FAILURE.
True  weld  thickness.    This  optional  value  is  available  for  solid
element failure, and is used to reduce the moment contribution to
the  failure  calculation  from  artificially  thick  weld  elements  under 
shear  loading  so  shear  failure  can  be  modeled  more  accurately.
See  comments  under  the  remarks  for  *MAT_SPOTWELD_DAIM-
LER CHRYSLER 
ASFF 
Weld assembly simultaneous failure flag 
EQ.0: Damaged elements fail individually. 
EQ.1: Damaged  elements 
fail  when 
first  reaches 
failure
criterion. 
BETA 
Damage model decay rate. 
DMGOPT 
Damage option flag.  If DMGOPT: 
EQ.0:  Plastic strain based damage. 
EQ.1:  Plastic  strain  based  damage  with  post  damage  stress
limit
VARIABLE   
DESCRIPTION
EQ.2:  Time based damage with post damage stress limit 
EQ.10:  Like  DMGOPT = 0,  but  failure  option  will  initiate 
damage 
EQ.11:  Like  DMGOPT = 1,  but  failure  option  will  initiate 
damage 
EQ.12:  Like  DMGOPT = 2,  but  failure  option  will  initiate 
damage 
FMODE 
Failure surface ratio for damage or failure, for DMGOPT = 10, 11, 
or 12 
EQ.0:  Damage initiates 
GT.0:  Damage or failure  
FFCAP 
Failure function limit for OPT = 0 or -1, and DMGOPT = 10, 11, or 
12  
EQ.0:  Damage initiates 
GT.0:  Damage or failure  
USRVn 
Failure  constants  for  OPT = 12  or  22  user  defined  failure, 
𝑛 = 7, 8, … , 22 
Weld Failure 
Spot  weld  material  is  modeled  with  isotropic  hardening  plasticity  coupled  to  failure 
models.    EFAIL  specifies  a  failure  strain  which  fails  each  integration  point  in  the  spot 
weld independently.  The OPT parameter is used to specify a failure criterion that fails 
the  entire  weld  element  when  the  criterion  is  met.    Alternatively,  EFAIL  and  OPT 
option may be used to initiate damage when the DAMAGE-FAILURE option is active 
using RS, BETA, and DMGOPT as described below. 
Beam  spot  weld  elements  can  use  any  OPT  value  except  7.    Brick  spot  weld  elements 
can use any OPT value except 3, 4, 5, 6, 9, and -9.  Hex assembly spot welds can use any 
OPT value except 9 and -9. 
OPT = -1 or 0 
OPT = 0 and OPT = -1 invoke a resultant-based failure criterion that fails the weld if the 
resultants are outside of the failure surface defined by: 
[
max(𝑁𝑟𝑟, 0)
𝑁𝑟𝑟𝐹
]
]
+ [
𝑁𝑟𝑠
𝑁𝑟𝑠𝐹
+ [
𝑁𝑟𝑡
𝑁𝑟𝑡𝐹
]
]
+ [
𝑀𝑟𝑟
𝑀𝑟𝑟𝐹
+ [
𝑀𝑠𝑠
𝑀𝑠𝑠𝐹
]
]
+ [
𝑀𝑡𝑡
𝑀𝑡𝑡𝐹
− 1 = 0
where  the  numerators    in  the  equation  are  the  resultants  calculated  in  the  local 
coordinates  of  the  cross  section,  and  the  denominators  are  the  values  specified  in  the 
input.    If  OPT = -1,  the  failure  surface  equation  is  evaluated,  but  element  failure  is 
suppressed.    This  allows  easy  identification  of  vulnerable  spot  welds  when  post-
processing.  Failure is likely to occur if FC > 1.0. 
Alternatively  a  *DEFINE_FUNCTION  could  be  used  to  define  the  Weld  Failure  for 
OPT = 0.  Then set FVAL = function ID.  Such a function could look like this: 
*DEFINE_FUNCTION 
        100 
 func(nrr,nrs,nrt,mrr,mss,mtt)= (nrr/5.0)*(nrr/5.0) 
The  six  arguments  for  this  function  (nrr,  …,  mtt)  are  the  force 
and moment resultants during the computation. 
OPT = 1: 
OPT = 1  invokes  a  stress  based  failure  model,  which  was  developed  by  Toyota  Motor 
Corporation and is based on the peak axial and transverse shear stresses.  The weld fails 
if the stresses are outside of the failure surface defined by 
(
𝜎𝑟𝑟
𝐹 )
𝜎𝑟𝑟
+ (
𝜏𝐹)
− 1 = 0 
If strain rates are considered then the failure criteria becomes: 
[
𝜎𝑟𝑟
]
𝐹 (𝜀̇eff)
𝜎𝑟𝑟
+ [
]
𝜏𝐹(𝜀̇eff)
− 1 = 0 
where  𝜎𝑟𝑟
stresses are calculated from the resultants using simple beam theory. 
𝐹 (𝜀̇eff)  and  𝜏𝐹(𝜀̇eff)  are  defined  by  load  curves  LCAX  and  LCTAU.    The  peak 
𝜎𝑟𝑟 =
𝑁𝑟𝑟
+
2 + 𝑀𝑡𝑡
√𝑀𝑠𝑠
2 + 𝑁𝑟𝑡
√𝑁𝑟𝑠
where the area and section modulus are given by: 
𝑀𝑟𝑟
2𝑍
𝜏 =
+
𝐴 = 𝜋
𝑍 = 𝜋
𝑑2
𝑑3
32
and  d  is  the  equivalent  diameter  of  the  beam  element  or  solid  element  used  as  a  spot 
weld.
*MAT_SPOTWELD 
OPT = 2 invokes a user-written subroutine uweldfail, documented in Appendix Q. 
OPT = 12 or 22 
OPT = 12  and  OPT = 22  invoke  similar  user-written  subroutines,  uweldfail12,  or, 
uweldfail22  respectively.  Both allow up to 22 failure parameters to be used rather than 
the 6 allowed with OPT = 2.  OPT = 12 also allows user control of weld damage. 
OPT = 3 
OPT = 3 invokes a failure based on notch stress, see Zhang [1999].  Failure occurs when 
the failure criterion: 
is satisfied.  The notch stress is given by the equation: 
𝜎𝑘 − 𝜎𝑘𝐹 ≥ 0 
𝜎𝑘 = 𝛼1
⎜⎛1 +
4𝐹
𝜋𝑑𝑡 ⎝
√3 + √19
8√𝜋
√
⎟⎞ + 𝛼2
𝜌⎠
6𝑀
𝜋𝑑𝑡2
⎜⎛1 +
⎝
√3𝜋
√
⎟⎞ + 𝛼3
𝜌⎠
4𝐹𝑟𝑟
𝜋𝑑2
⎜⎛1 +
⎝
3√2𝜋
√
⎟⎞ 
𝜌⎠
Here, 
𝐹 = √𝐹𝑟𝑠
2  
2 + 𝐹𝑟𝑡
𝑀 = √𝑀𝑠𝑠
2  
2 + 𝑀𝑡𝑡
and 𝛼𝑖    𝑖 = 1,2,3 are input corrections factors with default values of unity.  If spot welds 
are  between  sheets  of  unequal  thickness,  the  minimum  thickness  of  the  spot  welded 
sheets may be introduced as a crude approximation. 
OPT = 4 
OPT = 4  invokes  failure  based  on  structural stress  intensity,  see  Zhang  [1999].    Failure 
occurs when the failure criterion: 
is satisfied where 
and 
𝐾eq − 𝐾eqF ≥ 0 
𝐾eq = √𝐾𝐼
2  
2 + 𝐾𝐼𝐼
𝐾𝐼 = 𝛼1
√3𝐹
2𝜋𝑑√𝑡
+ 𝛼2
2√3𝑀
𝜋𝑑𝑡√𝑡
+ 𝛼3
5√2𝐹𝑟𝑟
3𝜋𝑑√𝑡
𝐾𝐼𝐼 = 𝛼1
2𝐹
𝜋𝑑√𝑡
Here,  F  and  M  are  as  defined  above  for  the  notch  stress  formulas  and  again,  𝛼𝑖    𝑖 =
1,2,3  are  input  corrections  factors  with  default  values  of  unity.    If  spot  welds  are 
between sheets of unequal thickness, the minimum thickness of the spot welded sheets 
may be used as a crude approximation. 
The maximum structural stress at the spot weld was utilized successfully for predicting 
the  fatigue  failure  of  spot  welds,  see  Rupp,  et.    al.  [1994]  and  Sheppard  [1993].    The 
corresponding results according to Rupp, et.  al.  are listed below where it is assumed 
that they may be suitable for crash conditions. 
OPT = 5 
OPT = 5 invokes failure by 
max(𝜎𝑣1, 𝜎𝑣2, 𝜎𝑣3) − 𝜎𝑠𝐹 = 0 
where 𝜎𝑠𝐹  is  the  critical  value  of  structural  stress  at  failure.    It  is  noted  that  the  forces 
and  moments  in  the  equations  below  are  referred  to  the  beam  nodes  1,  2,  and  to  the 
midpoint, respectively.  The three stress values, 𝜎𝑣1, 𝜎𝑣2, 𝜎𝑣3, are defined by: 
𝜎𝑣1(𝜁 ) =
𝐹𝑟𝑠1
𝜋𝑑𝑡1
cos𝜁 +
𝐹𝑟𝑡1
𝜋𝑑𝑡1
sin𝜁 −
1.046𝛽1𝐹𝑟𝑟1
𝑡1√𝑡1
−
1.123𝑀𝑠𝑠1
𝑑𝑡1√𝑡1
sin𝜁 +
1.123𝑀𝑡𝑡1
𝑑𝑡1√𝑡1
cos𝜁  
with  
𝛽1 = {
0 𝐹𝑟𝑟1 ≤ 0
1 𝐹𝑟𝑟1 > 0
𝜎𝑣2(𝜁 ) =
𝐹𝑟𝑠2
𝜋𝑑𝑡2
cos𝜁 +
𝐹𝑟𝑡2
𝜋𝑑𝑡2
sin𝜁 −
1.046𝛽1𝐹𝑟𝑟2
𝑡2√𝑡2
+
1.123𝑀𝑠𝑠2
𝑑𝑡2√𝑡2
sin𝜁 −
1.123𝑀𝑡𝑡2
𝑑𝑡2√𝑡2
cos𝜁  
with  
where 
𝛽2 = {
0 𝐹𝑟𝑟2 ≤ 0
1 𝐹𝑟𝑟2 > 0
𝜎𝑣3(𝜁 ) = 0.5𝜎(𝜁 ) + 0.5𝜎(𝜁 )cos(2𝛼) + 0.5𝜏(𝜁 )sin(2𝛼) 
𝜎(𝜁 ) =
𝜏(𝜁 ) =
𝛼 =
32𝑀𝑡𝑡
𝜋𝑑3 cos𝜁  
32𝑀𝑠𝑠
𝜋𝑑3 sin𝜁 −
16𝐹𝑟𝑡
3𝜋𝑑2 cos2𝜁  
4𝛽3𝐹𝑟𝑟
𝜋𝑑2 +
16𝐹𝑟𝑠
3𝜋𝑑2 sin2𝜁 +
tan−1 2𝜏(𝜁 )
𝜎(𝜁 )
𝛽3 = {
0 𝐹𝑟𝑟 ≤ 0
1 𝐹𝑟𝑟 > 0
The  stresses  are  calculated  for  all  directions,  0° ≤ 𝜁 ≤ 90°,  in  order  to  find  the 
maximum.  
OPT = 10 
OPT = 10 invokes the failure criterion developed by Lee and Balur (2011).  It is available 
for  welds  modeled  by  beam  elements,  solid  elements,  or  solid  assemblies.    A  detailed 
discussion  of  the  criterion  is  given  in  the  user’s  manual  section  for  *DEFINE_-
SPOTWELD_FAILURE. 
OPT = 11 
OPT = 11 invokes a resultant force based failure criterion for beams.  With correspond-
ing load curves or tables LCT and LCC, resultant force at failure 𝐹𝑓𝑎𝑖𝑙 can be defined as 
function of loading direction 𝛾 (curve ) or loading direction 𝛾 and effective strain rate 𝜀̇ 
(table): 
with the following definitions for loading direction (in degree) and effective strain rate: 
𝐹fail = 𝑓 (𝛾)      or     𝐹fail = 𝑓 (𝛾, 𝜀̇) 
𝛾 = tan−1 (∣
𝐹shear
𝐹axial
∣) ,      𝜀̇ = [
(𝜀̇axial
2 + 𝜀shear
2 ̇ )]
1/2
It  depends  on  the  sign  of  the  axial  beam  force,  if  LCT  or  LCC  are  used  for  failure 
condition: 
𝐹axial > 0:       [𝐹axial
2 + 𝐹shear
𝐹axial < 0:       [𝐹axial
2 + 𝐹shear
1/2
]
1/2
]
> Ffail,LCT     →     failure 
> Ffail,LCC     →     failure 
For  all  OPT  failure  criteria,  if  a  zero  is  input  for  a  failure  parameter  on  card  2,  the 
corresponding  term  will  be  omitted  from  the  equation.    For  example,  if  for  OPT = 0, 
only 𝑁𝑟𝑟𝐹 is nonzero, the failure surface is reduced to |𝑁𝑟𝑟| = 𝑁𝑟𝑟𝐹. 
Similarly, if the failure strain EFAIL is set to zero, the failure strain model is not used.  
Both EFAIL and OPT failure may be active at the same time. 
NF specifies the number of terms used to filter the stresses or resultants used in the OPT 
failure  criterion.    NF  cannot  exceed  30.    The  default  value  is  set  to  zero  which  is 
generally  recommended  unless  oscillatory  resultant  forces  are  observed  in  the  time 
history  databases.    Although  welds  should  not  oscillate  significantly,  this  option  was 
added for consistency with the other spot weld options.  NF affects the storage since it
is  necessary  to  store  the  resultant  forces  as  history  variables.    The  NF  parameter  is 
available only for beam element welds. 
The  inertias  of  the  spot  welds  are  scaled  during  the  first  time  step  so  that  their  stable 
time  step  size  is  Δ𝑡.    A  strong  compressive  load  on  the  spot  weld  at  a  later  time  may 
reduce the length of the spot weld so that stable time step size drops below Δ𝑡.  If the 
value  of  Δ𝑡  is  zero,  mass  scaling  is  not  performed,  and  the  spot  welds  will  probably 
limit  the  time  step  size.    Under  most  circumstances,  the  inertias  of  the  spot  welds  are 
small enough that scaling them will have a negligible effect on the structural response 
and the use of this option is encouraged. 
Spot weld force history data is written into the swforc ASCII file.  In this database the 
resultant  moments  are  not  available,  but  they  are  in  the  binary  time  history  database 
and in the ASCII elout file. 
Damage 
When  the  DAMAGE-FAILURE  option  is  invoked,  the  constitutive  properties  for  the 
damaged material are obtained from the undamaged material properties.  The amount 
of  damage  evolved  is  represented  by  the  constant,  𝜔,  which  varies  from  zero  if  no 
damage has occurred to unity for complete rupture.  For uniaxial loading, the nominal 
stress in the damaged material is given by  
𝜎nominal =
where P is the applied load and A is the surface area.  The true stress is given by:  
where 𝐴loss is the void area.  The damage variable can then be defined: 
𝜎true =
𝐴 − 𝐴loss
where, 
𝜔 =
𝐴loss
0 ≤ 𝜔 ≤ 1 
In this model, damage is initiated when the effective plastic strain in the weld exceeds 
the  failure  strain,  EFAIL.    If  DMGOPT = 10,  11,  or  12,  damage  will  initiate  when  the 
effective  plastic  strain  exceeds  EFAIL,  or  when  the  failure  criterion  is  met,  which  ever 
occurs first.  The failure criterion is specified by OPT parameter.  After damage initiates, 
the damage variable is evaluated by one of two ways. 
For  DMGOPT = 0,  1,  10,  or  11,  the  damage  variable  is  a  function  of  effective  plastic 
strain in the weld:
𝜀failure
≤ 𝜀eff
𝑝 ≤ 𝜀rupture
⇒ 𝜔 =
𝑝 − 𝜀failure
𝜀eff
− 𝜀failure
𝜀rupture
where 𝜀failure
a function of time: 
 = EFAIL and 𝜀rupture
 = RS.  For DMGOPT = 2 or 12, the damage variable is 
𝑡failure ≤ 𝑡 ≤ 𝑡rupture ⇒ 𝜔 =
𝑡 − 𝑡failure
𝑡rupture
where  𝑡failure  is  the  time  at  which  damage  initiates,  and  𝑡rupture = RS.    For  this  criteria, 
𝑝   exceeds  EFAIL,  or  the  time  when  the  failure 
𝑡failure  is  set  to  either  the  time  when  𝜀eff
criterion is met. 
For  DMGOPT = 1,  the  damage  behavior  is  the  same  as  for  DMGOPT = 0,  but  an 
additional  damage  variable  is  calculated  to  prevent  stress  growth  during  softening.  
Similarly, DMGOPT = 11 behaves like DMGOPT = 10 except for the additional damage 
variable.  This additional function is also used with DMGOPT = 2 and 12.  The effect of 
this  additional  damage  function  is  noticed  only  in  brick  and  brick  assembly  welds  in 
tension loading where it prevents growth of the tensile force in the weld after damage 
initiates. 
For DMGOPT = 10, 11, or 12 an optional FMODE parameter determines whether a weld 
that  reaches  the  failure  surface  will  fail  immediately,  or  initiate  damage.    The  failure 
surface calculation has shear terms, which may include the torsional moment, and also 
normal  and  bending  terms.      If  FMODE  is  input  with  a  value  between  0  and  1,  then 
when the failure surface is reached, the sum of  the square of the shear terms is divided 
by the sum of the square of all terms.  If this ratio exceeds FMODE, then the weld will 
fail immediately.  If the ratio is less than or equal to FMODE, then damage will initiate.  
The FMODE option is available only for brick and brick assembly welds.  
For  resultant  based  failure  (OPT = -1  or  0)  and  DMGOPT = 10,  11,  or  12  an  optional 
FFCAP  parameter  determines  whether  a  weld  that  reaches  the  failure  surface  will  fail 
immediately.  After damage initiation, the failure function can reach values above 1.0.  
This can now be limited by the FFCAP value (should be larger than 1.0): 
max(𝑁𝑟𝑟, 0)
]
𝑁𝑟𝑟𝐹
⎜⎛[
⎝
+ [
𝑁𝑟𝑠
𝑁𝑟𝑠𝐹
]
]
+ [
𝑁𝑟𝑡
𝑁𝑟𝑡𝐹
+ [
𝑀𝑟𝑟
𝑀𝑟𝑟𝐹
]
+ [
𝑀𝑠𝑠
𝑀𝑠𝑠𝐹
]
+ [
𝑀𝑡𝑡
𝑀𝑡𝑡𝐹
]
⎟⎞
⎠
< FFCAP 
BETA 
If  BETA  is  specified,  the  stress  is  multiplied  by  an  exponential  using  ω  defined  in  the 
previous equations,
𝜎𝑑 = 𝜎exp(−𝛽𝜔). 
For weld elements in an assembly ,  the  failure  criterion  is  evaluated  using  the 
assembly  cross  section.    If  damage  is  not  active,  all  elements  will be  deleted  when  the 
failure criterion is met.  If damage is active, then damage is calculated independently in 
each  element  of  the  assembly.    By  default,  elements  of  the  assembly  are  deleted  as 
damage  in  each  element  is  complete.    If  ASFF = 1,  then  failure  and  deletion  of  all 
elements  in  the  assembly  will  occur  simultaneously  when  damage  is  complete  in  any 
one of the elements. 
TRUE_T 
Weld elements and weld assemblies are tied to the mid-plane of shell materials and so 
typically  have  a  thickness  that  is  half  the  sum  of  the  thicknesses  of  the  welded  shell 
sections.  As a result, a weld under shear loading can be subject to an artificially large 
moment which will be balanced by normal forces transferred through the tied contact.  
These  normal  forces  will  cause  the  out-of-plane  bending  moment  used  in  the  failure 
calculation to be artificially high.  Inputting a TRUE_T that is smaller than the modeled 
thickness, for example, 10%-30% of true thickness will scale down the moment or stress 
that results from the balancing moment and provide more realistic failure calculations 
for solid elements and weld assemblies.  TRUE_T effects only the failure calculation, not 
the  weld  element  behavior.    If  TRUE_T = 0  or  data  is  omitted,  the  modeled  weld 
element thickness is used.  For OPT = 0, the two out-of-plane moments, 𝑀𝑠𝑠 and 𝑀𝑡𝑡 are 
replaced by modified terms 𝑀̂𝑠𝑠 and 𝑀̂𝑡𝑡, as shown below: 
[
max(𝑁𝑟𝑟, 0)
𝑁𝑟𝑟𝐹
]
]
+ [
𝑁𝑟𝑠
𝑁𝑟𝑠𝐹
+ [
𝑁𝑟𝑡
𝑁𝑟𝑡𝐹
]
]
+ [
𝑀𝑟𝑟
𝑀𝑟𝑟𝐹
+ [
𝑀̂𝑠𝑠
𝑀𝑠𝑠𝐹
]
]
+ [
𝑀̂𝑡𝑡
𝑀𝑡𝑡𝐹
− 1 = 0 
𝑀̂𝑠𝑠 = 𝑀𝑠𝑠 − 𝑁𝑟𝑡(𝑡 − 𝑡true) 
𝑀̂𝑡𝑡 = 𝑀𝑡𝑡 − 𝑁𝑟𝑠(𝑡 − 𝑡true) 
In  the  above,  𝑡  is  the  element  thickness  and  . 𝑡true  is  the  TRUE_T  parameter.    For 
OPT = 1,  the  same  modification  is  done  to  the  moments  that  contribute  to  the  normal 
stress, as shown below: 
𝜎𝑟𝑟 =
𝑁𝑟𝑟
+
√𝑀̂𝑠𝑠
2 + 𝑀̂
𝑡𝑡
Uniaxial option 
A uniaxial stress option is available for solid and solid weld assemblies.  It is invoked 
by defining the elastic modulus, 𝐸 as a negative number where the absolute value of 𝐸 
is the desired value for 𝐸.  The uniaxial option causes the two transverse stress terms to
be assumed to be zero throughout the calculation.  This assumption eliminates parasitic 
transverse stress that causes slow growth of plastic strain based damage. 
The motivation for this option can be explained with a weld loaded in tension.  Due to 
Poisson’s effect, an element in tension would be expected to contract in the transverse 
directions.  However, because the weld nodes are constrained to the mid-plane of shell 
elements,  such  contraction  is  only  possible  to  the  degree  that  that  shell  element 
contracts.  In other words, the uniaxial stress state cannot be represented by the weld.  
For  plastic  strain  based  damage,  this  effect  can  be  particularly  apparent  as  it  causes 
tensile  stress  to  continue  to  grow  very  large  as  the  stress  state  becomes  very  nearly 
triaxial tension.   In  this  stress  state,  plastic  strain  grows  very  slowly  so  it  appears that 
damage  calculation  is  failing  to  knock  down  the  stress.    By  simply  assuming  that  the 
transverse  stresses  are  zero,  the  plastic  strain  grows  as  expected  and  damage  is  much 
more effective. 
Material histories 
The probability of failure in solid or beam spotwelds can be estimated by retrieving the 
corresponding material histories for output to the d3plot database 
*DEFINE_MATERIAL_HISTORIES Properties 
Label 
Attributes 
Description 
Instability 
Damage 
- 
- 
- 
- 
- 
- 
-  A  measure  between  0  and  1  related  to 
how close the spotweld element is to fail 
-  Damage 
in 
the 
spotweld 
element 
between 0 and 1 
These  two  labels  are  supported  for  all  options  (OPT  and  DMGOPT,  including 
assemblies  and  beams),  except  for  user  defined  failure.    The  instability  measure  is  the 
maximum  over  time;  namely,  it  gives  the  maximum  value  for  a  given  element 
throughout the simulation.  If a damage option is invoked then damage will initiate and 
increment  when  the  instability  reaches  unity,  and  elements  are  not  deleted  until  the 
damage value reaches unity.  If no damage option is invoked then the damage output is 
always  zero  and  elements  will  be  deleted  at  the  point  when  the  instability  measure 
reaches unity.
*MAT_SPOTWELD_DAIMLERCHRYSLER 
This is Material Type 100.  The material model applies only to solid element type l.  If 
hourglass  type  4  is  specified  then  hourglass  type  4  will  be  used,  otherwise,  hourglass 
type 6 will be automatically assigned.  Hourglass type 6 is preferred. 
constraint 
Spot weld elements may be placed between any two deformable shell surfaces and tied 
*CONTACT_TIED_SURFACE_TO_SURFACE,  which 
with 
eliminates the need to have adjacent nodes at spot weld locations.  Spot weld failure is 
modeled using this card and *DEFINE_CONNECTION_PROPERTIES data.  Details of 
the failure model can be found in Seeger, Feucht, Frank, Haufe, and Keding [2005]. 
contact, 
NOTE:  It is advisable to include all spot welds, which pro-
vide  the  slave  nodes,  and  spot  welded  materials, 
which  define  the  master  segments,  within  a  single 
*CONTACT_TIED_SURFACE_TO_SURFACE  inter-
face.  This contact type uses constraint equations.  If 
multiple  interfaces  are  treated  independently,  sig-
nificant  problems  can  occur  if  such  interfaces  share 
common  nodes.    An  added  benefit  is  that  memory 
usage  can  be  substantially  less  with  a  single  inter-
face 
. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
Variable 
EFAIL 
Type 
F 
2 
RO 
F 
2 
3 
E 
F 
3 
4 
PR 
F 
4 
5 
6 
5 
6 
7 
DT 
F 
7 
8 
TFAIL 
F 
8 
NF
Card 3 
Variable 
1 
RS 
2 
3 
4 
5 
6 
7 
8 
ASFF 
TRUE_T 
CON_ID 
JTOL 
Type 
F 
I 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
DT 
TFAIL 
EFAIL 
NF 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
Time step size for mass scaling, Δ𝑡. 
Failure time if nonzero.  If zero this option is ignored. 
Effective  plastic  strain  in  weld  material  at  failure.    See  remark
below. 
Number  of  failure  function  evaluations  stored  for  filtering  by
time averaging.  The default value is set to zero which is generally
recommended  unless  oscillatory  resultant  forces  are  observed  in
the time history databases.  Even though these welds should not 
oscillate significantly, this option was added for consistency with
the  other  spot  weld  options.    NF  affects  the  storage  since  it  is
necessary  to  store  the  failure  terms.    When  NF  is  nonzero,  the
resultants in the output databases are filtered.  NF cannot exceed 
30. 
RS 
ASFF 
Rupture strain.  See Remarks below. 
Weld assembly simultaneous failure flag 
EQ.0: Damaged elements fail individually. 
EQ.1: Damaged  elements  fail  when  first  reaches  failure
criterion. 
TRUE_T 
True  weld  thickness  for  single  hexahedron  solid  weld  elements. 
See comments below.
DESCRIPTION
Connection  ID  of  *DEFINE_CONNECTION  card.    A  negative 
CON_ID deactivates failure, see comments below. 
Tolerance value for relative volume change (default: JTOL = 0.01). 
Solid  element  spotwelds  with  a  Jacobian  less  than  JTOL  will  be
eroded.  
  VARIABLE   
CON_ID 
JTOL 
Remarks: 
This weld material is modeled with isotropic hardening plasticity.  The yield stress and 
constant  hardening  modulus  are  assumed  to  be  those  of  the  welded  shell  elements  as 
defined  in  a  *DEFINE_CONNECTION_PROPERTIES  table.    A  failure  function  and 
damage  type  is  also  defined  by  *DEFINE_CONNECTION_PROPERTIES  data.    The 
interpretation  of  EFAIL  and  RS  is  determined  by  the  choice  of  damage  type.    This  is 
discussed in remark 4 on *DEFINE_CONNECTION_PROPERTIES. 
Solid weld elements are tied to the mid-plane of shell materials and so typically have a 
thickness that is half the sum of the thicknesses of the welded shell sections.  As a result, 
a weld under shear loading can be subject to an artificially large moment which will be 
balanced  by  normal  forces  transferred  through  the  tied  contact.    These  normal  forces 
will cause the normal term in the failure calculation to be artificially high.  Inputting a 
TRUE_T  that  is  smaller  than  the  modeled  thickness,  for  example,  10%-30%  of  true 
thickness will scale down the normal force that results from the balancing moment and 
provide more realistic failure calculations.  TRUE_T effects only the failure calculation, 
not  the  weld  element  behavior.    If  TRUE_T = 0  or  data  is  omitted,  the  modeled  weld 
element thickness is used. 
For weld elements in an assembly ,  the  failure  criterion  is  evaluated  using  the 
assembly  cross  section.    If  damage  is  not  active,  all  elements  will be  deleted  when  the 
failure criterion is met.  If damage is active, then damage is calculated independently in 
each  element  of  the  assembly.    By  default,  elements  of  the  assembly  are  deleted  as 
damage  in  each  element  is  complete.    If  ASFF = 1,  then  failure  and  deletion  of  all 
elements  in  the  assembly  will  occur  simultaneously  when  damage  is  complete  in  any 
one of the elements. 
Solid element force resultants for MAT_SPOTWELD are written to the spot weld force 
file,  swforc,  and  the  file  for  element  stresses  and  resultants  for  designated  elements, 
ELOUT.  Also, spot weld failure data is written to the file, dcfail. 
An  option  to  deactivate  weld  failure  is  switched  on  by  setting  CON_ID  to  a  negative 
value  where  the  absolute  value  of  CON_ID  becomes  the  connection  ID.    When  weld
failure is deactivated, the failure function is evaluated and output to swforc and dcfail 
but the weld retains its full strength.
*MAT_101 
is  Material  Type  101. 
This 
  The  GEPLASTIC_SRATE_2000a  material  model 
characterizes  General  Electric's  commercially  available  engineering  thermoplastics 
subjected to high strain rate events.  This material model features the variation of yield 
stress  as  a  function  of  strain  rate,  cavitation  effects  of  rubber  modified  materials  and 
automatic element deletion of either ductile or brittle materials. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
E 
F 
3 
4 
5 
6 
7 
8 
PR 
RATESF 
EDOT0 
ALPHA 
F 
4 
F 
5 
F 
6 
F 
7 
8 
Variable 
LCSS 
LCFEPS 
LCFSIG 
LCE 
Type 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young's Modulus. 
Poisson's ratio. 
RATESF 
Constant in plastic strain rate equation. 
EDOT0 
Reference strain rate 
ALPHA 
Pressure sensitivity factor 
LCSS 
Load  curve  ID  or  Table  ID  that  defines  the  post  yield  material
behavior.   The values of this stress-strain curve are the difference 
of  the  yield  stress  and  strain  respectively.    This  means  the  first
values for both stress  and strain should be zero.  All subsequent 
values will define softening or hardening.
Load curve ID that defines the plastic failure strain as a function
of strain rate. 
Load curve ID that defines the Maximum principal  failure stress
as a function of strain rate. 
Load curve ID that defines the Unloading moduli as a function of
plastic strain. 
*MAT_101 
  VARIABLE   
LCFEPS 
LCFSIG 
LCE 
Remarks: 
The constitutive model for this approach is: 
𝜀̇𝑝 = 𝜀̇0exp{𝐴[𝜎 − 𝑆(𝜀𝑝)]} × exp(−𝑝𝛼𝐴) 
where  𝜀̇0  and  A  are  rate  dependent  yield  stress  parameters,  𝑆(𝜀𝑝)  internal  resistance 
(strain hardening) and 𝛼  is a pressure dependence parameter. 
In  this  material  the  yield  stress  may  vary  throughout  the  finite  element  model  as  a 
function of strain rate and hydrostatic stress.  Post yield stress behavior is captured in 
material softening and hardening values.  Finally, ductile or brittle failure measured by 
plastic  strain  or  maximum  principal  stress  respectively  is  accounted  for  by  automatic 
element deletion. 
Although  this  may  be  applied  to  a  variety  of  engineering  thermoplastics,  GE  Plastics 
have  constants  available  for  use  in  a  wide  range  of  commercially  available  grades  of 
their engineering thermoplastics.
*MAT_INV_HYPERBOLIC_SIN_{OPTION}  
This  is  Material  Type  102.    It  allows  the  modeling  of  temperature  and  rate  dependent 
plasticity, Sheppard and Wright [1979]. 
Available options include: 
<BLANK> 
THERMAL 
such that the keyword card can appear as: 
*MAT_INV_HYPERBOLIC_SIN or *MAT_102 
*MAT_INV_HYPERBOLIC_SIN_THERMAL or *MAT_102_T 
Card 1 for <BLANK> option: 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
Card 2 for <BLANK> option: 
  Card 2 
1 
Variable 
ALPHA 
Type 
F 
2 
N 
F 
3 
E 
F 
3 
A 
F 
Card 1 for THERMAL option: 
  Card 1 
1 
2 
3 
Variable 
MID 
RO 
ALPHA 
Type 
A8 
F 
F 
4 
PR 
F 
4 
Q 
F 
4 
N 
F 
5 
T 
F 
5 
G 
F 
5 
A 
F 
8 
6 
HC 
F 
7 
VP 
F 
6 
7 
8 
EPS0 
LCQ 
F 
I 
6 
Q 
F 
7 
G 
F 
8 
EPSO
*MAT_INV_HYPERBOLIC_SIN 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCE 
LCPR 
LCCTE 
Type 
F 
F 
F 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
E 
PR 
T 
HC 
VP 
Mass density. 
Young’s Modulus. 
Poisson’s ratio 
Initial Temperature. 
Heat generation coefficient. 
Formulation for rate effects: 
EQ.0.0: Scale yield stress (default) 
EQ.1.0: Viscoplastic formulation. 
ALPHA 
α, see  Remarks.    Not  to  be  confused  with  coefficient  of  thermal
expansion. 
N 
A 
Q 
G 
EPS0 
LCQ 
See Remarks. 
See Remarks. 
See Remarks. 
See Remarks. 
Minimum strain rate considered in calculating Z. 
ID of curve specifying parameter Q. 
GT.0:  Q as function of plastic strain. 
LT.0:  Q as function of temperature.
VARIABLE   
DESCRIPTION
ID of curve defining Young’s Modulus vs.  temperature. 
ID of curve defining  Poisson’s ratio vs.  temperature. 
ID  of  curve  defining  coefficient  of  thermal  expansion  vs.
temperature. 
LCE 
LCPR 
LCCTE 
Remarks: 
Resistance  to  deformation  is  both  temperature  and  strain  rate  dependent.    The  flow 
stress equation is: 
𝜎 =
sinh−1
⎡
⎢
⎣
(
)
⎤
⎥
⎦
where 𝑍, the Zener-Holloman temperature compensated strain rate, is: 
𝑍 = max(𝜀̇,EPS0) × exp (
GT
) 
The  units  of  the  material  constitutive  constants  are  as  follows:  𝐴  (1/sec),  𝑁  
(dimensionless), 𝛼 (1/MPa), the activation energy for flow, 𝑄(J/mol), and the universal 
gas constant, 𝐺 (J/mol K).  The value of 𝐺 will only vary with the unit system chosen.  
Typically it will be either 8.3144 J/mol ∞ K, or 40.8825 lb in/mol ∞ R. 
The final equation necessary to complete our description of high strain rate deformation 
is one that allows us to compute the temperature change during the deformation.  In the 
absence  of  a  couples  thermo-mechanical  finite  element  code  we  assume  adiabatic 
temperature  change  and  follow  the  empirical  assumption  that  90-95%  of  the  plastic 
work is dissipated as heat.  Thus the heat generation coefficient is 
where 𝜌 is the density of the material and 𝐶𝑣 is the specific heat.
HC ≈
0.9
𝜌𝐶𝑣
*MAT_ANISOTROPIC_VISCOPLASTIC 
This is Material Type 103.  This anisotropic-viscoplastic material model applies to shell 
and  brick  elements.    The  material  constants  may  be  fit  directly  or,  if  desired,  stress 
versus strain data may be input and a least squares fit will be performed by LS-DYNA 
to  determine  the  constants.    Kinematic  or  isotopic  or  a  combination  of  kinematic  and 
isotropic hardening may be used.  A detailed description of this model can be found in 
the  following  references:  Berstad,  Langseth,  and  Hopperstad  [1994];  Hopperstad  and 
Remseth [1995]; and Berstad [1996].  Failure is based on effective plastic strain or by a 
user defined subroutine. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
E 
F 
3 
4 
PR 
F 
4 
5 
6 
7 
8 
SIGY 
FLAG 
LCSS 
ALPHA 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
QR1 
CR1 
QR2 
CR2 
QX1 
CX1 
QX2 
CX2 
Type 
F 
  Card 3 
Variable 
1 
VK 
Type 
F 
  Card 4 
1 
F 
2 
F 
3 
F 
4 
F 
5 
VM 
R00 or F  R45 or G  R90 or H 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
L 
F 
6 
F 
7 
M 
F 
7 
F 
8 
N 
F 
8 
Variable 
AOPT 
FAIL 
NUMINT 
MACF 
Type 
F 
F 
F
Variable 
1 
XP 
Type 
F 
  Card 6 
Variable 
1 
V1 
Type 
F 
2 
YP 
F 
2 
V2 
F 
3 
ZP 
F 
3 
V3 
F 
4 
A1 
F 
4 
D1 
F 
5 
A2 
F 
5 
D2 
F 
6 
A3 
F 
6 
D3 
F 
  VARIABLE   
DESCRIPTION
*MAT_103 
7 
8 
7 
8 
BETA 
F 
MID 
RO 
E 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus 
Poisson’s ratio 
SIGY 
Initial yield stress
FLAG 
Flag 
*MAT_ANISOTROPIC_VISCOPLASTIC 
DESCRIPTION
EQ.0: Give all material parameters 
EQ.1: Material parameters parameters 𝑄𝑟1, 𝐶𝑟1, 𝑄𝑟2, and 𝐶𝑟2 for 
pure  isotropic  hardening  (𝛼 = 1)  are  determined  by  a 
least  squares  fit  to  the  curve  or  table  specified  by  the
variable  LCSS.   If 𝛼  is  input  as  less  than  1,   𝑄𝑟1 and  𝑄𝑟2
are  then  modified  by  multiplying  them  by  the  factor  𝛼, 
while the factors 𝑄𝑥1 and 𝑄𝑥2 are taken as the product of 
the  original  parameters  𝑄𝑟1and  𝑄𝑟2,  resp.,  for  pure  iso-
tropic hardening and the factor (1 − 𝛼).  𝐶𝑥1 is set equal 
to 𝐶𝑟1 and 𝐶𝑥2 is set equal to 𝐶𝑟2.   𝛼 is input as variable 
ALPHA on Card 1 in columns 71-80. 
EQ.2: Use load curve directly, i.e., no fitting is required for the
parameters 𝑄𝑟1, 𝐶𝑟1, 𝑄𝑟2, and 𝐶𝑟2.  A table is not allowed 
and only isotropic hardening is implemented.  
EQ.4: Use  table  definition  directly,  no  fitting  is  required  and
the values for 𝑄𝑟1, 𝐶𝑟1, 𝑄𝑟2, 𝐶𝑟2, 𝑉𝑘, and 𝑉𝑚 are ignored. 
Only  isotropic  hardening  is  implemented,  and  this  op-
tion is only available for solids. 
LCSS 
Load curve ID or Table ID. 
Case  1:  LCSS  is  a  Load  Curve  ID.    The  load  curve  ID  defines 
effective  stress  versus  effective  plastic  strain.    Card  2  is  ignored 
with  this  option.    For  this  load  curve  case  viscoplasticity  is
modeled when the coefficients 𝑉𝑘 and 𝑉𝑚  are provided. 
Case  2:  LCSS  is  a  Table  ID.    Table  consists  of  stress  versuses 
effective  plastic  strain  curves  indexed  by  strain  rate.    See  Figure 
M24-1. 
FLAG.EQ.1:  Table  is  used  to  calculate  the  coefficients  𝑉𝑘  and 
𝑉𝑚. 
FLAG.EQ.4:  Table  is  interpolated  and  used  directly.    This
option is available only for solid elements. 
ALPHA 
𝛼  distribution  of  hardening  used  in  the  curve-fitting.  𝛼 = 0  pure 
kinematic hardening and 𝛼 = 1 provides pure isotropic hardening
QR1 
CR1 
Isotropic hardening parameter 𝑄𝑟1 
Isotropic hardening parameter 𝐶𝑟1
VARIABLE   
DESCRIPTION
QR2 
CR2 
QX1 
CX1 
QX2 
CX2 
VK 
VM 
R00 
R45 
R90 
F 
G 
H 
L 
M 
N 
Isotropic hardening parameter 𝑄𝑟2 
Isotropic hardening parameter 𝐶𝑟2 
Kinematic hardening parameter 𝑄𝜒1 
Kinematic hardening parameter 𝐶𝜒1 
Kinematic hardening parameter 𝑄𝜒2 
Kinematic hardening parameter 𝐶𝜒2 
Viscous material parameter 𝑉𝑘 
Viscous material parameter 𝑉𝑚 
𝑅00 for shell (Default = 1.0) 
𝑅45 for shell (Default = 1.0) 
𝑅90 for shell (Default = 1.0) 
𝐹 for brick (Default = 1/2) 
𝐺 for brick (Default = 1/2) 
𝐻 for brick (Default = 1/2) 
𝐿 for brick (Default = 3/2) 
𝑀 for brick (Default = 3/2) 
𝑁  for brick (Default = 3/2)
AOPT 
*MAT_ANISOTROPIC_VISCOPLASTIC 
DESCRIPTION
Material axes option : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES, and then, for shells only, rotated about
the shell element normal by an angle BETA. 
EQ.1.0: locally orthotropic with material axes determined by a
point  in  space  and  the  global  location  of  the  element
center;  this  is  the  a-direction.    This  option  is  for  solid 
elements only. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the 
element normal. 
EQ.4.0: locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector  v,  and
an originating point, P, which define the centerline ax-
is.  This option is for solid elements only. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
FAIL 
Failure flag. 
LT.0.0:  User  defined  failure  subroutine  is  called  to  determine 
failure.    This  is  subroutine  named,  MATUSR_103,  in 
dyn21.f. 
EQ.0.0: Failure is not considered.  This option is recommended
if failure is not of interest since many calculations will
be saved. 
GT.0.0:  Plastic strain to failure.  When the plastic strain reaches 
this value, the element is deleted from the calculation.
VARIABLE   
NUMINT 
DESCRIPTION
Number  of  integration  points  which  must  fail  before  element
deletion.  If zero, all points must fail.  This option applies to shell
elements only.  For the case of one point shells, NUMINT should
be set to a value that is less than the number of through thickness
integration points.  Nonphysical stretching can sometimes appear
in  the  results  if  all  integration  points  have  failed  except  for  one
point  away  from  the  midsurface.    This  is  due  to  the  fact  that
unconstrained  nodal  rotations  will  prevent  strains 
from
developing at the remaining integration point.  In fully integrated
shells, similar problems can occur. 
MACF 
Material axes change flag for brick elements: 
EQ.1: No change, default, 
EQ.2: switch material axes 𝑎 and 𝑏, 
EQ.3: switch material axes 𝑎 and 𝑐, 
EQ.4: switch material axes 𝑏 and 𝑐. 
XP, YP, ZP 
𝑥𝑝, 𝑦𝑝, 𝑧𝑝, define coordinates of point 𝐩 for AOPT = 1 and 4. 
A1, A2, A3 
𝑎1, 𝑎2, 𝑎3, define components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
𝑣1, 𝑣2, 𝑣3 define components of vector 𝐯 for AOPT = 3 and 4. 
D1, D2, D3 
𝑑1, 𝑑2, 𝑑3, define components of vector 𝐝 for AOPT = 2. 
BETA 
Material  angle  in  degrees  for  AOPT = 0  (shells  only)  and 
AOPT = 3.      BETA  may  be  overridden  on  the  element  card,  see
*ELEMENT_SHELL_BETA and *ELEMENT_SOLID_ORTHO.  
Remarks: 
The uniaxial stress-strain curve is given on the following form 
𝜎(𝜀eff
𝑝 , 𝜀̇eff
𝑝 ) = 𝜎0 + 𝑄𝑟1[(1 − exp(−𝐶𝑟1𝜀eff
+ 𝑄𝜒1[(1 − exp(−𝐶𝜒1𝜀eff
𝑝 ))] + 𝑄𝑟2[1 − exp(−𝐶𝑟2𝜀eff
𝑝 ))] + 𝑄𝜒2[(1 − exp(−𝐶𝜒2𝜀eff
𝑝 )]
𝑝 ))] + 𝑉𝑘𝜀̇eff
𝑝 𝑉𝑚 
For bricks the following yield criteria is used 
𝐹(𝜎22 − 𝜎33)2 + 𝐺(𝜎33 − 𝜎11)2 + 𝐻(𝜎11 − 𝜎22)2 + 2𝐿𝜎23
𝑝 )]
= [𝜎(𝜀eff
𝑝 , 𝜀̇eff
2 + 2𝑀𝜎31
2 + 2𝑁𝜎12
𝑝     is  the  effective  plastic  strain  and  𝜀̇eff
𝑝   is  the  effective  plastic  strain  rate.    For 
where 𝜀eff
shells the anisotropic behavior is given by 𝑅00, 𝑅45 and 𝑅90.  The model will work when 
the  three  first  parameters  in  card  3  are  given  values.    When  𝑉𝑘 = 0  the  material  will 
behave elasto-plastically.  Default values are given by: 
𝐹 = 𝐺 = 𝐻 =
𝐿 = 𝑀 = 𝑁 =
𝑅00 = 𝑅45 = 𝑅90 = 1 
Strain rate of accounted for using the Cowper and Symonds model which, e.g., model 3, 
scales the yield stress with the factor: 
⎜⎛
⎝
To  convert  these  constants  set  the  viscoelastic  constants,  𝑉𝑘  and  𝑉𝑚,  to  the  following 
values: 
1   +   
𝑝⁄
𝜀̇eff
⎟⎞
𝐶 ⎠
)
𝑉𝑘 = (
𝑉𝑚 =
If  LCSS  is  nonzero,  substitute  the  initial,  quasi-static  yield  stress  for  SIGY  in  the 
equation for 𝑉𝑘  above. 
This model properly treats rate effects.  The viscoplastic rate formulation is an option in 
other  plasticity  models  in  LS-DYNA,  e.g.,  mat_3  and  mat_24,  invoked  by  setting  the 
parameter VP to 1.
*MAT_103_P 
This  is  Material  Type  103_P.    This  anisotropic-plastic  material  model  is  a  simplified 
version  of  the  MAT_ANISOTROPIC_VISCOPLASTIC  above.    This  material  model 
applies only to shell elements. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
E 
F 
3 
4 
PR 
F 
4 
Variable 
QR1 
CR1 
QR2 
CR2 
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
F 
4 
5 
6 
7 
8 
SIGY 
LCSS 
F 
5 
F 
6 
7 
8 
5 
6 
7 
8 
Variable 
R00 
R45 
R90 
S11 
S22 
S33 
S12 
Type 
F 
  Card 4 
1 
Variable 
AOPT 
Type 
F 
  Card 5 
Variable 
1 
XP 
Type 
F 
F 
2 
2 
YP 
F 
F 
3 
3 
ZP 
F 
F 
4 
4 
A1 
F 
F 
5 
5 
A2 
F 
F 
6 
6 
A3 
F 
F 
7 
8 
7
Card 6 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
7 
8 
BETA 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
SIGY 
LCSS 
QR1 
CR1 
QR2 
CR2 
R00 
R45 
R90 
S11 
S22 
S33 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus 
Poisson’s ratio 
Initial yield stress 
Load curve ID.  The load curve ID defines effective stress versus
effective plastic strain.  Card 2 is ignored with this option. 
Isotropic hardening parameter 𝑄𝑟1 
Isotropic hardening parameter 𝐶𝑟1 
Isotropic hardening parameter 𝑄𝑟2 
Isotropic hardening parameter 𝐶𝑟2 
𝑅00 for anisotropic hardening 
𝑅45 for anisotropic hardening 
𝑅90 for anisotropic hardening 
Yield  stress  in  local  𝑥-direction.    This  input  is  ignored  if 
(𝑅00, 𝑅45, 𝑅90) > 0. 
Yield  stress  in  local  𝑦-direction.    This  input  is  ignored  if 
(𝑅00, 𝑅45, 𝑅90) > 0. 
Yield  stress  in  local  𝑧-direction.    This  input  is  ignored  if 
(𝑅00, 𝑅45, 𝑅90) > 0.
VARIABLE   
DESCRIPTION
S12 
AOPT 
Yield  stress  in  local    -direction.    This  input  is  ignored  if 
(𝑅00, 𝑅45, 𝑅90) > 0. 
Material axes option : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES,  and  then  rotated  about  the  shell  ele-
ment normal by an angle BETA. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by 
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the
element normal. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
XP, YP, ZP 
𝑥𝑝, 𝑦𝑝, 𝑧𝑝 define coordinates of point 𝐩 for AOPT = 1 and 4. 
A1, A2, A3 
𝑎1, 𝑎2, 𝑎3 define components of vector 𝐚 for AOPT = 2. 
D1, D2, D3 
𝑑1, 𝑑2, 𝑑3 define components of vector 𝐝 for AOPT = 2. 
V1, V2, V3 
𝑣1, 𝑣2, 𝑣3 define components of vector 𝐯 for AOPT = 3 and 4. 
BETA 
Material angle in degrees for AOPT = 0 and 3, may be overridden 
on the element card, see *ELEMENT_SHELL_BETA. 
Remarks: 
If  no  load  curve  is  defined  for  the  effective  stress  versus  effective  plastic  strain,  the 
uniaxial stress-strain curve is given on the following form 
𝜎(𝜀eff
𝑝 ) = 𝜎0 + 𝑄𝑟1[1 − exp(−𝐶𝑟1𝜀eff
𝑝 )] + 𝑄𝑟2[1 − exp(−𝐶𝑟2𝜀eff
𝑝 )]
𝑝  is the effective plastic strain.  For shells the anisotropic behavior is given by 
where 𝜀eff
𝑅00, 𝑅45 and 𝑅90, or the yield stress in the different direction.  Default values are given 
by: 
if the variables R00, R45, R90, S11, S22, S33 and S12 are set to zero.
𝑅00 = 𝑅45 = 𝑅90 = 1
*MAT_104 
This is Material Type 104.  This is a continuum damage mechanics (CDM) model which 
includes  anisotropy  and  viscoplasticity.    The  CDM  model  applies  to  shell,  thick  shell, 
and  brick  elements.    A  more  detailed  description  of  this  model  can  be  found  in  the 
paper by Berstad, Hopperstad, Lademo, and Malo [1999].  This material model can also 
model anisotropic damage behavior by setting the FLAG to -1 in Card 2. 
3 
E 
F 
3 
Q2 
F 
3 
4 
PR 
F 
4 
C2 
F 
4 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
2 
C1 
F 
2 
  Card 2 
Variable 
1 
Q1 
Type 
F 
  Card 3 
Variable 
1 
VK 
Type 
F 
  Card 4 
1 
VM 
R00 or  F R45 or G  R90 or H 
F 
2 
F 
3 
F 
4 
Variable 
AOPT 
CPH 
MACF 
Type 
F 
F 
I 
5 
6 
7 
8 
SIGY 
LCSS 
LCDS 
F 
5 
6 
7 
8 
EPSD 
S or EPSR 
DC 
FLAG 
F 
5 
F 
5 
Y0 
F 
F 
6 
L 
F 
6 
F 
7 
M 
F 
7 
F 
8 
N 
F 
8 
ALPHA 
THETA 
ETA 
F 
F
Variable 
1 
XP 
Type 
F 
  Card 6 
Variable 
1 
V1 
Type 
F 
2 
YP 
F 
2 
V2 
F 
3 
ZP 
F 
3 
V3 
F 
4 
A1 
F 
4 
D1 
F 
5 
A2 
F 
5 
D2 
F 
6 
A3 
F 
6 
D3 
F 
*MAT_DAMAGE_1 
7 
8 
7 
8 
BETA 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
SIGY 
LCSS 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s modulus 
Poisson’s ratio 
Initial yield stress, 𝜎0 
Load  curve  ID  defining  effective  stress  versus  effective  plastic
strain.    Isotropic  hardening  parameters  on  Card  2  are  ignored
with this option. 
LCDS 
Load curve ID defining nonlinear damage curve.  For FLAG = -1. 
Q1 
C1 
Q2 
C2 
EPSD 
S 
Isotropic hardening parameter 𝑄1 
Isotropic hardening parameter 𝐶1 
Isotropic hardening parameter 𝑄2 
Isotropic hardening parameter 𝐶2 
Damage  threshold  𝜀eff,d
material softening begins.  (Default = 0.0) 
.    Damage  effective  plastic  strain  when 
Damage material constant 𝑆. (Default =  
𝜎0
200).  For FLAG ≥ 0.
VARIABLE   
DESCRIPTION
EPSR 
DC 
Effective  plastic  strain  at  which  material  ruptures  (logarithmic).
For FLAG = -1. 
Critical damage value 𝐷𝐶. When the damage value 𝐷 reaches this 
value, the element is deleted from the calculation.  (Default = 0.5) 
For FLAG ≥ 0. 
FLAG 
Flag 
EQ.-1:  Anisotropic damage 
EQ.0:  Standard isotropic damage (default) 
EQ.1:  Standard  isotropic  damage  plus  strain  localization
check (only for shell elements) 
EQ.10: Enhanced isotropic damage  
EQ.11: Enhanced  isotropic  damage  plus  strain  localization
check (only for shell elements) 
VK 
VM 
R00 
R45 
R90 
F 
G 
H 
L 
M 
N 
Viscous material parameter 𝑉𝑘 
Viscous material parameter 𝑉𝑚 
𝑅00 for shell (Default = 1.0) 
𝑅45 for shell (Default = 1.0) 
𝑅90 for shell (Default = 1.0) 
F for brick (Default = 1/2) 
G for brick (Default = 1/2) 
H for brick (Default = 1/2) 
L for brick (Default = 3/2) 
M for brick (Default = 3/2) 
N for brick (Default = 3/2) 
AOPT 
Material  axes  option  : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES, and then, for shells only, rotated about
*MAT_DAMAGE_1 
DESCRIPTION
the shell element normal by an angle BETA. 
EQ.1.0: locally orthotropic with material axes determined by a
point  in  space  and  the  global  location  of  the  element
center;  this  is  the  a-direction.    This  option  is  for  solid 
elements only. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element 
defined  by  the  cross  product  of  the  vector  v  with  the
element normal. 
EQ.4.0: locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector  v,  and
an originating point, P, which define the centerline ax-
is.  This option is for solid elements only. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
CPH 
Microdefects  closure  parameter  h 
(FLAG ≥ 10). 
for  enhanced  damage 
MACF 
Material axes change flag for brick elements: 
EQ.1: No change, default, 
EQ.2: switch material axes a and b, 
EQ.3: switch material axes a and c, 
EQ.4: switch material axes b and c. 
Y0 
Initial  damage  energy  release  rate  Y0  for  enhanced  damage 
(FLAG ≥ 10). 
ALPHA 
Exponent 𝛼 for enhanced damage (FLAG ≥ 10) 
THETA 
Exponent 𝜃 for enhanced damage (FLAG ≥ 10) 
ETA 
Exponent 𝜂 for enhanced damage (FLAG ≥ 10)
VARIABLE   
DESCRIPTION
XP, YP, ZP 
𝑥𝑝, 𝑦𝑝, 𝑧𝑝: define coordinates of point 𝐩 for AOPT = 1 and 4 
A1, A2, A3 
𝑎1, 𝑎2, 𝑎3: define components of vector 𝐚 for AOPT = 2 
D1, D2, D3 
𝑑1, 𝑑2, 𝑑3: define components of vector 𝐝 for AOPT = 2 
V1, V2, V3 
𝑣1, 𝑣2, 𝑣3: define components of vector 𝐯 for AOPT = 3 and 4 
BETA 
Μaterial  angle  in  degrees  for  AOPT = 0  (shells  only)  and 
AOPT = 3.      BETA  may  be  overridden  on  the  element  card,  see
*ELEMENT_SHELL_BETA and *ELEMENT_SOLID_ORTHO. 
Remarks: 
Standard  isotropic  damage  model  (FLAG   =   0  or  1).  The  Continuum  Damage 
Mechanics  (CDM)  model  is  based  on  an  approach  proposed  by  Lemaitre  [1992].    The 
effective stress 𝜎̃ , which is the stress calculated over the section that effectively resist the 
forces, reads 
𝜎̃ =
1 − 𝐷
where  𝐷  is  the  damage  variable.    The  evolution  equation  for  the  damage  variable  is 
defined as 
𝐷̇ =
⎧ 0
{
⎨
{
⎩
 𝜀̇eff
for
for
𝑝 ≤ 𝜀eff,d
𝜀eff
𝑝 > 𝜀eff,d
𝜀eff
and 𝜎1 > 0
where 𝜀eff,d
𝜎1 is the maximum principal stress.  The damage energy density release rate is  
 is the damage threshold, 𝑆 is the so-called damage energy release rate and 
𝑌 =
𝐞𝐞: 𝐂: 𝐞𝐞 =
2 𝑅𝑣
𝜎𝑣𝑚
2𝐸(1 − 𝐷)2 
where 𝐸 is Young’s modulus and 𝜎𝑣𝑚 is the equivalent von Mises stress.  The triaxiality 
function 𝑅𝑣 is defined as  
𝑅𝑣 =
(1 + 𝜈) + 3(1 − 2𝜈) (
𝜎𝐻
𝜎𝑣𝑚
)
with Poisson’s ratio 𝜈 and hydrostatic stress 𝜎𝐻. 
Enhanced isotropic damage model (FLAG  =  10 or 11). A more sophisticated damage 
model  including  crack  closure  effects  (reduced  damage  under  compression)  and  more 
flexibility  in  stress  state  dependence  and  functional  expressions  is  invoked  by  setting
FLAG = 10  or  11.    The  corresponding  evolution  equation  for  the  damage  variable  is 
defined as 
𝐷̇ = (
2𝜏max
𝜎𝑣𝑚
)
 ⟨
𝑌 − 𝑌0
⟩
𝑝  
 (1 − 𝐷)1−𝜃 𝜀̇eff
where  𝜏max  is  the  maximum  shear  stress,  𝑌0  is  the  initial  damage  energy  release  rate 
and  𝜂,  𝛼,  and  𝜃  are  additional  material  constants.  〈 〉  are  the  Macauley  brackets.    The 
damage energy density release rate is  
𝑌 =
1 + 𝜈
2𝐸
(∑(〈𝜎̃𝑖〉2 + ℎ〈−𝜎̃𝑖〉2)
) −
𝑖=1
2𝐸
(〈𝜎̃𝐻〉2 + ℎ〈−𝜎̃𝐻〉2) 
where 𝜎̃𝑖 are the principal effective stresses and h is the microdefects closure parameter 
that  accounts  for  different  damage  behavior  in  tension  and  compression.    A  value  of 
ℎ ≈ 0.2  is  typically  observed  in  many  experiments  as  stated  in  Lemaitre  [2000].    A 
parameter  set  of ℎ = 1,  𝑌0 = 0,  𝛼 = 1,  𝜃 = 1,  and  𝜂 = 0  should  give  the  same  results  as 
the standard isotropic damage model (FLAG = 0/1) with 𝜀eff,d
= 0 as long as 𝜎1 > 0. 
Strain  localization  check  (FLAG  =  1  or  11).  In  order  to  add  strain  localization 
computation  to  the  damage  models  above,  parameter  FLAG  should  be  set  to  1 
(standard  damage)  or  11  (enhanced  damage).    An  acoustic  tensor  based  bifurcation 
criterion  is  checked  and  history  variable  no.    4  is  set  to  1.0  if  strain  localization  is 
indicated.  Only available for shell elements. 
Anisotropic  damage  model  (FLAG = -1).  At  each  thickness  integration  points,  an 
anisotropic damage law acts on the plane stress tensor in the directions of the principal 
total shell strains, 𝜀1 and 𝜀2, as follows: 
𝜎11 = [1 − 𝐷1(𝜀1)]𝜎110 
𝜎22 = [1 − 𝐷2(𝜀2)]𝜎220 
𝜎12 = [1 −
𝐷1 + 𝐷2
] 𝜎120 
The transverse plate shear stresses in the principal  strain directions are assumed to be 
damaged as follows: 
𝜎13 = (1 − 𝐷1/2)𝜎130 
𝜎23 = (1 − 𝐷2/2)𝜎230 
In  the  anisotropic  damage  formulation,  𝐷1(𝜀1)  and  𝐷2(𝜀2)  are  anisotropic  damage 
functions  for  the  loading  directions  1  and  2,  respectively.    Stresses  𝜎110, 𝜎220,𝜎120, 𝜎130 
and  𝜎230  are  stresses  in  the  principal  shell  strain  directions  as  calculated  from  the 
undamaged elastic-plastic material behavior.  The strains 𝜀1 and 𝜀2 are the magnitude of 
the principal strains calculated upon reaching the damage thresholds.  Damage can only 
develop for tensile stresses, and the damage functions 𝐷1(𝜀1) and 𝐷2(𝜀2)are identical to 
zero  for  negative  strains  𝜀1  and  𝜀2.  The  principal  strain  directions  are  fixed  within  an 
integration point as soon as either principal strain exceeds the initial threshold strain in
tension.  A more detailed description of the damage evolution for this material model is 
given in the description of Material 81. 
Anisotropic  viscoplasticity.  The  uniaxial  stress-strain  curve  is  given  in  the  following 
form 
𝜎(𝑟, 𝜀̇eff
𝑝 ) = 𝜎0 + 𝑄1[1 − exp(−𝐶1𝑟)] + 𝑄2[1 − exp(−𝐶2𝑟)] + 𝑉𝑘𝜀̇eff
𝑝 𝑉𝑚 
where r is the damage accumulated plastic strain, which can be calculated by 
𝑟 ̇ = 𝜀̇eff
For bricks the following yield criterion associated with the Hill criterion is used 
𝑝 (1 − 𝐷) 
𝐹(𝜎̃22 − 𝜎̃33)2 + 𝐺(𝜎̃33 − 𝜎̃11)2 + 𝐻(𝜎̃11 − 𝜎̃22)2 + 2𝐿𝜎̃23
2 + 2𝑀𝜎̃31
2 + 2𝑁𝜎̃12
2 = 𝜎(𝑟, 𝜀̇eff
𝑝 ) 
𝑝   is  the  effective  viscoplastic 
where  𝑟  is  the  damage  effective  viscoplastic  strain  and  𝜀̇eff
strain  rate.    For  shells  the  anisotropic  behavior  is  given  by  the  R-values:  𝑅00,  𝑅45,  and 
𝑅90.    When  𝑉𝑘 = 0  the  material  will  behave  as  an  elastoplastic  material  without  rate 
effects.  Default values for the anisotropic constants are given by: 
𝐹 = 𝐺 = 𝐻 =
𝐿 = 𝑀 = 𝑁 =
𝑅00 = 𝑅45 = 𝑅90 = 1 
so that isotropic behavior is obtained. 
Strain  rate  is  accounted  for  using  the  Cowper  and  Symonds  model  which  scales  the 
yield stress with the factor: 
1 + (
𝑝⁄
)
𝜀̇
To  convert  these  constants,  set  the  viscoelastic  constants,  𝑉𝑘  and  𝑉𝑚,  to  the  following 
values: 
𝑉𝑘 = 𝜎 (
)
𝑉𝑚 =
F 
0 
8 
*MAT_105 
*MAT_DAMAGE_2 
*MAT_DAMAGE_2 
This is Material Type 105.  This is an elastic viscoplastic material model combined with 
continuum damage mechanics (CDM).  This material model applies to shell, thick shell, 
and  brick  elements.    The  elastoplastic  behavior  is  described  in  the  description  of 
material  model  24.    A  more  detailed  description  of  the  CDM  model  is  given  in  the 
description of material model 104 above. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
6 
7 
8 
SIGY 
ETAN 
FAIL 
TDEL 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
0.0 
10.E+20 
  Card 2 
Variable 
Type 
Default 
1 
C 
F 
0 
  Card 3 
1 
Variable 
EPSD 
Type 
F 
2 
P 
F 
0 
2 
S 
F 
3 
4 
5 
6 
7 
LCSS 
LCSR 
F 
0 
4 
F 
0 
3 
DC 
F 
5 
6 
7 
8 
Default 
none 
none 
none
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EPS1 
EPS2 
EPS3 
EPS4 
EPS5 
EPS6 
EPS7 
EPS8 
Type 
Default 
F 
0 
  Card 5 
1 
F 
0 
2 
F 
0 
3 
F 
0 
4 
F 
0 
5 
F 
0 
6 
F 
0 
7 
F 
0 
8 
Variable 
ES1 
ES2 
ES3 
ES4 
ES5 
ES6 
ES7 
ES8 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
SIGY 
ETAN 
FAIL 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
Yield stress. 
Tangent modulus, ignored if (LCSS.GT.0) is defined. 
Failure flag. 
EQ.0.0: Failure due to plastic strain is not considered. 
GT.0.0: Plastic strain to failure.  When the plastic strain reaches
this value, the element is deleted from the calculation. 
TDEL 
Minimum time step size for automatic element deletion. 
C 
P 
Strain rate parameter, C, see formula below. 
Strain rate parameter, P, see formula below.
LCSS 
LCSR 
EPSD 
S 
DC 
*MAT_DAMAGE_2 
DESCRIPTION
Load  curve  ID  or  Table  ID.    Load  curve  ID  defining  effective
stress  versus  effective  plastic  strain.    If  defined  EPS1 -  EPS8  and 
ES1 -  ES8  are  ignored.      The  table  ID  defines  for  each  strain  rate
value  a  load  curve  ID  giving  the  stress  versus  effective  plastic
strain for that rate, See Figure M24-1.  The stress versus effective 
plastic strain curve for the lowest value of strain rate is used if the
strain  rate  falls  below  the  minimum  value.    Likewise,  the  stress
versus effective plastic strain curve for the highest value of strain
rate  is  used  if  the  strain  rate  exceeds  the  maximum  value.    The
strain rate parameters: C and P; the curve ID, LCSR; EPS1 - EPS8 
and ES1 - ES8 are ignored if a Table ID is defined. 
Load curve ID defining strain rate scaling effect on yield stress. 
Damage  threshold  𝑟𝑑  Damage  effective  plastic  strain  when 
material softening begin.  (Default = 0.0) 
Damage material constant 𝑆. (Default =
𝜎0
200) 
Critical  damage  value  𝐷𝐶.    When  the  damage  value  𝐷  reaches 
this  value, 
the  calculation. 
(Default = 0.5) 
the  element 
is  deleted 
from 
EPS1 - EPS8 
Effective  plastic  strain  values  (optional  if  SIGY  is  defined).    At
least 2 points should be defined. 
ES1 - ES8 
Corresponding yield stress values to EPS1 - EPS8. 
Remarks: 
The  stress-strain  behavior  may  be  treated  by  a  bilinear  curve  by  defining  the  tangent 
modulus, ETAN.  Alternately, a curve similar to that shown in Figure M10-1 is expected 
to  be  defined  by  (EPS1,ES1)  -  (EPS8,ES8);  however,  an  effective  stress  versus  effective 
plastic strain curve ID (LCSS) may be input instead if eight points are insufficient.  The 
cost is roughly the same for either approach.  The most general approach is to use the 
table definition with table ID, LCSR, discussed below. 
Three options to account for strain rate effects are possible. 
1.  Strain rate may be accounted for using the Cowper and Symonds model which 
scales the yield stress with the factor 
1 + (
𝑝⁄
)
𝜀̇
where 𝜀̇ is the strain rate, 𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗 
2.  For  complete  generality  a  load  curve  (LCSR)  to  scale  the  yield  stress  may  be 
input instead.  In this curve the scale factor versus strain rate is defined. 
3. 
If different stress versus strain curves can be provided for various strain rates, 
the  option  using  the  reference  to  a  table  (LCSS)  can  be  used.    Then  the  table 
input in *DEFINE_TABLE has to be used, see Figure M24-1 
A fully viscoplastic formulation is used in this model.
*MAT_ELASTIC_VISCOPLASTIC_THERMAL 
This is Material Type 106.  This is an elastic viscoplastic material with thermal effects. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
E 
F 
3 
4 
PR 
F 
4 
5 
6 
7 
8 
SIGY 
ALPHA 
LCSS 
FAIL 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
QR1 
CR1 
QR2 
CR2 
QX1 
CX1 
QX2 
CX2 
Type 
F 
  Card 3 
Variable 
Type 
1 
C 
F 
  Card 4 
1 
F 
2 
P 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
LCE 
LCPR 
LCSIGY 
LCR 
LCX 
LCALPH 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
LCC 
LCP 
TREF 
LCFAIL 
Type 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus 
Poisson’s ratio
VARIABLE   
DESCRIPTION
SIGY 
LCSS 
Initial yield stress 
Load  curve  ID  or  Table  ID.    The  load  curve  ID  defines  effective
stress versus effective plastic strain.  The table ID defines for each
temperature  value  a  load  curve  ID  giving  the  stress  versus
effective  plastic  strain  for  that  temperature  (DEFINE_TABLE)  or 
it defines for each temperature value a table ID which defines for
each strain rate a load curve ID giving the stress versus effective
plastic  strain  (DEFINE_TABLE_3D).    The  stress  versus  effective 
plastic  strain  curve  for  the  lowest  value  of  temperature  or  strain 
rate  is  used  if  the  temperature  or  strain  rate  falls  below  the
minimum value.  Likewise, maximum values cannot be exceeded.
Card 2 is ignored with this option.   
FAIL 
Effective plastic failure strain for erosion.  
ALPHA 
Coefficient of thermal expansion. 
QR1 
CR1 
QR2 
CR2 
QX1 
CX1 
QX2 
CX2 
C 
P 
LCE 
Isotropic hardening parameter 𝑄𝑟1 
Isotropic hardening parameter 𝐶𝑟1 
Isotropic hardening parameter 𝑄𝑟2 
Isotropic hardening parameter 𝐶𝑟2 
Kinematic hardening parameter 𝑄𝜒1 
Kinematic hardening parameter 𝐶𝜒1 
Kinematic hardening parameter 𝑄𝜒2 
Kinematic hardening parameter 𝐶𝜒2 
Viscous material parameter 𝐶 
Viscous material parameter 𝑃 
Load  curve  defining  Young's  modulus  as  a  function  of
temperature. 
E on card 1 is ignored with this option. 
LCPR 
Load curve defining Poisson's ratio as a function of temperature.
PR on card 1 is ignored with this option.
LCSIGY 
*MAT_ELASTIC_VISCOPLASTIC_THERMAL 
DESCRIPTION
Load  curve  defining  the  initial  yield  stress  as  a  function  of
temperature.  SIGY on card 1 is ignored with this option. 
LCR 
LCX 
Load  curve  for  scaling  the  isotropic  hardening  parameters  QR1
and QR2  or the stress given by the load curve LCSS as a function
of temperature. 
Load  curve  for  scaling  the  kinematic  hardening  parameters  QX1
and QX2 as a function of temperature. 
LCALPH 
Load  curve  ID  defining  the  instantaneous  coefficient  of  thermal
expansion as a function of temperature: 
𝑑𝜀𝑖𝑗
thermal = 𝛼(𝑇)𝑑𝑇𝛿𝑖𝑗 
ALPHA  on  card  1  is  ignored  with  this  option.    If  LCALPH  is
defined as the negative of the load curve ID, the curve is assumed
to define the coefficient relative to a reference temperature, TREF
below, such that the total thermal strain is give by 
thermal = 𝛼(𝑇)(𝑇 − 𝑇ref)𝛿𝑖𝑗
𝜀𝑖𝑗
LCC 
LCP 
TREF 
Load  curve  for  scaling  the  viscous  material  parameter  C  as  a
function of temperature. 
Load  curve  for  scaling  the  viscous  material  parameter  P  as  a
function of temperature. 
Reference  temperature  required  if  and  only  if  LCALPH  is  given 
with a negative curve ID. 
LCFAIL 
Load  curve  defining  the  plastic  failure  strain  as  a  function  of
temperature.  FAIL on card 1 is ignored with this option. 
Remarks: 
If LCSS is not given any value the uniaxial stress-strain curve has the form 
𝑝 )]
𝑝 )] + 𝑄𝜒2[1 − exp(−𝐶𝜒2𝜀eff
𝑝 ) = 𝜎0 + 𝑄𝑟1[1 − exp(−𝐶𝑟1𝜀eff
𝑝 )] + 𝑄𝑟2[1 − exp(−𝐶𝑟2𝜀eff
+ 𝑄𝜒1[1 − exp(−𝐶𝜒1𝜀eff
𝜎(𝜀eff
𝑝 )] 
Viscous effects are accounted for using the Cowper and Symonds model, which scales 
the yield stress with the factor:
1 +
𝑝⁄
.
𝜀̇eff
⎟⎞
𝐶 ⎠
⎜⎛
⎝
*MAT_MODIFIED_JOHNSON_COOK 
This  is  Material  Type  107.    Adiabatic  heating  is  included  in  the  material  formulation.  
Material type 107 is not intended for use in a coupled thermal-mechanical analysis or in 
a mechanical analysis where temperature is prescribed using *LOAD_THERMAL.     
Define the following two cards with general material parameters 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
Variable 
E0DOT 
Type 
F 
2 
RO 
F 
2 
Tr 
F 
3 
E 
F 
3 
Tm 
F 
4 
PR 
F 
4 
T0 
F 
5 
6 
BETA 
XS1 
F 
5 
F 
6 
FLAG1 
FLAG2 
F 
F 
7 
CP 
F 
7 
8 
ALPHA 
F 
8 
Card 3 for Modified Johnson-Cook Constitutive Relation.  This format is used when 
FLAG1 = 0. 
  Card 3 
Variable 
Type 
1 
A 
F 
2 
B 
F 
3 
N 
F 
4 
C 
F 
5 
m 
F 
6 
7 
8 
Card 4 for Modified Johnson-Cook Constitutive Relation.  This format is used when 
FLAG1 = 0. 
  Card 4 
Variable 
1 
Q1 
Type 
F 
2 
C1 
F 
3 
Q2 
F 
4 
C2 
F 
5 
6 
7
Card  3  for  Modified  Zerilli-Armstrong  Constitutive  Relation.    This  format  is  used 
when FLAG1 = 1. 
  Card 3 
1 
Variable 
SIGA 
Type 
F 
2 
B 
F 
3 
4 
5 
6 
7 
8 
BETA0 
BETA1 
F 
F 
Card  4  for  Modified  Zerilli-Armstrong  Constitutive  Relation.    This  format  is  used 
when FLAG1 = 1. 
  Card 4 
Variable 
Type 
1 
A 
F 
2 
N 
F 
3 
4 
5 
6 
7 
8 
ALPHA0 
ALPHA1 
F 
F 
Card  5  for  Modified  Johnson-Cook  Fracture  Criterion.    This  format  is  used  when 
FLAG2 = 0. 
  Card 5 
Variable 
1 
DC 
Type 
F 
2 
PD 
F 
3 
D1 
F 
4 
D2 
F 
5 
D3 
F 
6 
D4 
F 
7 
D5 
F 
8 
Card  5  for  Cockcroft  Latham  Fracture  Criterion.    This  format  is  used  when 
FLAG2 = 1. 
3 
4 
5 
6 
7 
8 
  Card 5 
Variable 
1 
DC 
2 
WC 
Type 
F
Additional Element Erosion Criteria Card. 
  Card 6 
Variable 
1 
TC 
2 
3 
4 
5 
6 
7 
8 
TAUC 
Type 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s modulus, E. 
Poisson’s ratio, 𝑣. 
BETA 
Damage coupling parameter; see Eq.  (107.3). 
EQ.0.0: No  coupling  between  ductile  damage  and 
the 
constitutive relation. 
EQ.1.0: Full  coupling  between  ductile  damage  and 
the
constitutive relation. 
Taylor-Quinney coefficient 𝜒, see Eq.  (107.20).  Gives the portion 
of plastic work converted into heat (normally taken to be 0.9) 
Specific heat 𝐶𝑝, see Eq.  (107.20) 
XS1 
CP 
ALPHA 
Thermal expansion coefficient, 𝛼. 
EPS0 
Tr 
Tm 
T0 
Quasi-static 
EQ.(107.12).Set description under *MAT_015. 
threshold 
strain 
rate 
(𝜀̇0 = 𝑝̇0 = 𝑟 ̇0), 
see 
Room temperature, see Eq.  (107.13) 
Melt temperature, see Eq.  (107.13) 
Initial temperature
VARIABLE   
DESCRIPTION
FLAG1 
Constitutive relation flag; see Eq.  (107.11) and (107.14) 
EQ.0.0: Modified  Johnson-Cook  constitutive  relation,  see  Eq. 
(107.11). 
EQ.1.0: Zerilli-Armstrong 
(107.14). 
constitutive 
relation, 
see  Eq.
FLAG2 
Fracture criterion flag; see Eq.  (107.15) and (107.19). 
EQ.0.0: Modified  Johnson-Cook  fracture  criterion;  see  Eq. 
(107.15). 
EQ.1.0: Cockcroft-Latham fracture criterion; see Eq.  (107.19). 
K 
G 
A 
B 
N 
C 
M 
Q1 
C1 
Q2 
C2 
Bulk modulus 
Shear modulus 
Johnson-Cook yield stress A, see Eq.  (107.11). 
Johnson-Cook hardening parameter B, see Eq.  (107.11). 
Johnson-Cook hardening parameter n, see Eq.  (107.11). 
Johnson-Cook  strain  rate  sensitivity  parameter  C,  see  Eq.
(107.11). 
Johnson-Cook thermal softening parameter m, see Eq.  (107.11). 
Voce hardening parameter 𝑄1 (when B = n = 0), see Eq.  (107.11). 
Voce hardening parameter 𝐶1 (when B = n = 0), see Eq.  (107.11). 
Voce hardening parameter 𝑄2 (when B = n = 0), see Eq.  (107.11). 
Voce hardening parameter 𝐶2 (when B = n = 0), see Eq.  (107.11). 
SIGA 
B 
BETA0 
BETA1 
Zerilli-Armstrong parameter 𝛼𝑎, see Eq.  (107.14). 
Zerilli-Armstrong parameter 𝐵, see Eq.  (107.14). 
Zerilli-Armstrong parameter 𝛽0, see Eq.  (107.14). 
Zerilli-Armstrong parameter 𝛽1, see Eq.  (107.14). 
A 
Zerilli-Armstrong parameter 𝐴, see Eq.  (107.14).
*MAT_MODIFIED_JOHNSON_COOK 
DESCRIPTION
N 
Zerilli-Armstrong parameter 𝑛, see Eq.  (107.14). 
ALPHA0 
Zerilli-Armstrong parameter 𝛼0, see Eq.  (107.14). 
ALPHA1 
Zerilli-Armstrong parameter 𝛼1, see Eq.  (107.14). 
DC 
Critical  damage  parameter  𝐷𝑐,  see  Eq.    (107.15)  and  (107.21). 
When  the  damage  value  𝐷  reaches  this  value,  the  element  is 
eroded from the calculation. 
PD 
Damage threshold, see Eq.  (107.15). 
D1-D5 
Fracture  parameters  in  the  Johnson-Cook  fracture  criterion,  see 
Eq.  (107.16). 
Critical Cockcroft-Latham parameter 𝑊𝑐, see Eq.  (107.19).  When 
the  plastic  work  per  volume  reaches  this  value,  the  element  is
eroded from the simulation. 
Critical  temperature  parameter  𝑇𝑐,  see  Eq.    (107.23).    When  the 
temperature 𝑇, reaches this value, the element is eroded from the
simulation. 
Critical  shear  stress  parameter  𝜏𝑐.    When  the  maximum  shear 
stress  𝜏  reaches  this  value,  the  element  is  eroded  from  the
simulation. 
WC 
TC 
TAUC 
Remarks: 
An additive decomposition of the rate-of-deformation tensor 𝐝 is assumed, i.e. 
𝐝 = 𝐝𝑒 + 𝐝𝑝 + 𝐝𝑡
(107.1)
Where 𝐝𝑒 is the elastic part, 𝐝𝑝 is the plastic part and 𝐝𝑡 is the thermal part. 
The elastic rate-of-deformation 𝐝𝑒 is defined by a linear hypo-elastic relation 
σ̃∇𝐽 = (𝐾 −
𝐺) tr(𝐝𝑒)𝐈 + 𝟐𝐺𝐝𝑒
(107.2)
Where  𝐈  is  the  unit  tensor, 𝐾  is  the  bulk  modulus  and  𝐺  is  the  shear  modulus.    The 
effective stress tensor is defined by 
σ̃ =
1 − 𝛽𝐷
(107.3)
Where σ is the Cauchy-stress and 𝐷 is the damage variable, while the Jaumann rate of 
the effective stress reads 
σ̃∇𝐽 = σ̃̇ − 𝐖 ⋅ σ̃ − σ̃ ⋅ 𝐖𝑇
(107.4)
Where  𝐖  is  the  spin  tensor.    The  parameter  𝛽  is  equal  to  unity  for  coupled  damage 
and equal to zero for uncoupled damage. 
The thermal rate-of-deformation 𝐝𝑇 is defined by 
𝐝𝑇 = 𝛼𝑇̇𝐈
Where 𝛼 is the linear thermal expansion coefficient and 𝑇 is the temperature. 
The plastic rate-of-deformation is defined by the associated flow rule as 
𝐝𝑝 = 𝑟 ̇
∂𝑓
∂σ
=
𝑟 ̇
1 − 𝛽𝐷
σ̃′
𝜎̃eq
(107.5)
(107.6)
Where (⋅)′ means the deviatoric part of the tensor, 𝑟 is the damage-equivalent plastic 
strain, 𝑓  is the dynamic yield function, i.e. 
𝐝𝑝 = 𝑟 ̇
∂𝑓
∂σ
=
𝑟 ̇
1 − 𝛽𝐷
σ̃′
𝜎̃eq
And 𝜎̃eq is the damage-equivalent stress. 
σ̃′: σ̃′ − 𝜎𝑌(𝑟, 𝑟 ̇, 𝑇) ≤ 0,
𝑓 = √
𝑟 ̇ ≥ 0,
𝑟 ̇𝑓 = 0 
𝜎̃eq = √
σ̃′: σ̃′
The following plastic work conjugate pairs are identified 
𝑊̇ 𝑝 = σ: 𝐝𝑝 = 𝜎̃eq𝑟 ̇ = 𝜎eq𝑝̇
(107.6)
(107.7)
(107.8)
(107.9)
Where  𝑊̇ 𝑝  is  the  specific  plastic  work  rate,  and  the  equivalent  stress  𝜎eq  and  the 
equivalent plastic strain 𝑝 are defined as  
𝜎eq = √
σ̃′: σ̃′ = (1 − 𝛽𝐷)𝜎̃eq 𝑝̇ = √
𝐝𝑝: 𝐝𝑝 =
𝑟 ̇
(1 − 𝛽𝐷)
(107.10)
The material strength 𝜎𝑌 is defined by: 
1.  The modified Johnson-Cook constitutive relation 
𝜎𝑌 = {𝐴 + 𝐵𝑟𝑛 + ∑ 𝑄𝑖[1 − exp(−𝐶𝑖𝑟)]
𝑖=1
} (1 + 𝑟 ̇∗)𝐶(1 − 𝑇∗𝑚) 
(107.11)
Where 𝐴, 𝐵, 𝐶, 𝑚, 𝑛, 𝑄1, 𝐶1, 𝑄2, 𝐶2 are material parameters; the normalized dam-
age-equivalent plastic strain rate 𝑟 ̇∗ is defined by  
𝑟 ̇∗ =
𝑟 ̇
𝜀̇0
(107.12)
In which 𝜀̇0 is a user-defined reference strain rate; and the homologous temper-
ature reads 
𝑇∗ =
𝑇 − 𝑇𝑟
𝑇𝑚 − 𝑇𝑟
(107.13)
In which 𝑇𝑟 is the room temperature and 𝑇𝑚 is the melting temperature. 
2.  The Zerilli-Armstrong constitutive relation 
𝜎𝑌 = {𝜎𝑎 + 𝐵exp[−(𝛽0 − 𝛽1ln𝑟 ̇)𝑇] + 𝐴𝑟𝑛exp[−(𝛼0 − 𝛼1ln𝑟 ̇)𝑇]} 
(107.14)
Where 𝜎𝑎, 𝐵, 𝛽0, 𝛽1, 𝐴, 𝑛, 𝛼0, 𝛼1 are material parameters. 
Damage evolution is defined by: 
1.  The extended Johnson-Cook damage evolution rule: 
𝐷̇ =
𝐷𝑐
𝑝𝑓 − 𝑝𝑑
⎧
{
⎨
{
⎩
𝑝 ≤ 𝑝𝑑
𝑝 > 𝑝𝑑
(107.15)
Where the current equivalent fracture strain 𝑝𝑓 = 𝑝𝑓 (𝜎 ∗, 𝑝̇∗, 𝑇∗) is defined as 
𝑝𝑓 = [𝐷1 + 𝐷2exp(𝐷3𝜎 ∗)](1 + 𝑝̇∗)𝐷4(1 + 𝐷5𝑇∗)
(107.16)
and  𝐷1, 𝐷2, 𝐷3,  𝐷4,  𝐷5,  𝐷𝐶,  𝑝𝑑  are  material  parameters;  the  normalized 
equivalent plastic strain rate 𝑝̇∗ is defined by 
𝑝̇∗ =
𝑝̇
𝜀̇0
and the stress triaxiality 𝜎 ∗ reads 
𝜎 ∗ =
𝜎𝐻
𝜎eq
,
𝜎𝐻 =
𝑡𝑟(σ)
2.The Cockcroft-Latham damage evolution rule: 
𝐷̇ =
𝐷𝐶
𝑊𝐶
max(𝜎1, 0)𝑝̇
where 𝐷𝐶, 𝑊𝐶 are material parameters. 
(107.17)
(107.18)
(107.19)
Adiabatic heating is calculated as  
𝑇̇ = 𝜒
𝛔: 𝐝𝑝
𝜌𝐶𝑝
= 𝜒
𝜎̃𝑒𝑞𝑟 ̇
𝜌𝐶𝑝
(107.20)
Where 𝜒 is the Taylor-Quinney parameter, 𝜌 is the density and 𝐶𝑝 is the specific heat.  
The initial value of the temperature 𝑇0 may be specified by the user. 
Element erosion occurs when one of the following several criteria are fulfilled: 
1.  The damage is greater than the critical value 
𝐷 ≥ 𝐷𝐶
(107.21)
2.  The maximum shear stress is greater than a critical value 
𝜏max =
max{|𝜎1 − 𝜎2|, ∣𝜎2 − 𝜎3∣, ∣𝜎3 − 𝜎1∣} ≥ 𝜏𝐶
(107.22)
3.  The temperature is greater than a critical value 
𝑇 ≥ 𝑇𝐶
(107.23)
History Variable 
Description 
1 
2 
3 
4 
5 
8 
9 
Evaluation of damage D 
Evaluation of stress triaxiality 𝜎 ∗ 
Evaluation of damaged plastic strain r 
Evaluation of temperature T 
Evaluation of damaged plastic strain rate 𝑟 ̇ 
Evaluation of plastic work per volume W 
Evaluation of maximum shear stress 𝜏max
*MAT_ORTHO_ELASTIC_PLASTIC 
This  is  Material  Type  108.    This  model  combines  orthotropic  elastic  plastic  behavior 
with an anisotropic yield criterion.  This model is implemented only for shell elements. 
  Card  1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
  Card  2 
1 
Variable 
SIGMA0 
Type 
F 
  Card  3 
1 
2 
LC 
I 
2 
3 
4 
5 
6 
7 
8 
E11 
E22 
G12 
PR12 
PR23 
PR31 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
QR1 
CR1 
QR2 
CR2 
F 
3 
F 
4 
F 
5 
F 
6 
7 
8 
Variable 
R11 
R22 
R33 
R12 
Type 
F 
  Card  4 
1 
F 
2 
Variable 
AOPT 
BETA 
Type 
F 
F 
  Card  5 
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
F 
3 
3 
ZP 
F 
F 
4 
4 
A1 
F 
5 
6 
7 
8 
7 
8 
5 
A2 
F 
6 
A3
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
D17 
F 
5 
D2 
F 
6 
D3 
F 
  VARIABLE   
DESCRIPTION
*MAT_108 
7 
8 
MID 
RO 
E11 
E22 
G12 
PR12 
PR23 
PR31 
LC 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass Density 
Young’s Modulus in 11-direction 
Young’s Modulus in 22-direction 
Shear modulus in 12-direction 
Poisson’s ratio 12 
Poisson’s ratio 23 
Poisson’s ratio 31 
Load curve ID.  This curve defines effective stress versus effective
plastic  strain.    QR1,  CR1,  QR2,  and  CR2  are  ignored  if  LC  is
defined.   
SIGMA0 
Initial yield stress, 𝜎0 
QR1 
CR1 
QR2 
CR2 
R11 
R22 
R33 
R12 
Isotropic hardening parameter, 𝑄𝑅1 
Isotropic hardening parameter, 𝐶𝑅1 
Isotropic hardening parameter, 𝑄𝑅2 
Isotropic hardening parameter, 𝐶𝑅2 
Yield criteria parameter, 𝑅11 
Yield criteria parameter, 𝑅22 
Yield criteria parameter, 𝑅33 
Yield criteria parameter, 𝑅12
AOPT 
*MAT_ORTHO_ELASTIC_PLASTIC 
DESCRIPTION
Material  axes  option   
EQ.0.0: Locally  orthotropic  with  material  axes  determined  by
element  nodes  as  shown  in  Figure  M2-1.    Nodes  1,  2 
and  4  of  an  element  are  identical  to  the  node  used  for
the definition of a coordinate system as by *DEFINE_-
COORDINATE_NODES,  and  then  rotated  about  the 
shell element normal by an angle BETA.   
EQ.2.0: Globally orthotropic with material axes determined by 
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: Locally  orthotropic  material  axes  determined  by
offsetting the material axes by an angle, BETA, from a
line determined by taking the cross product of the vec-
tor v with the normal to the plane of the element. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
BETA 
Material  angle  in  degrees  for  AOPT = 0  and  3.    BETA  may  be 
overridden on the element card, see *ELEMENT_SHELL_BETA.  
XP YP ZP 
Coordinates of point 𝐩 for AOPT = 1. 
A1 A2 A3 
Components of vector 𝐚 for AOPT = 2. 
V1 V2 V3 
Components of vector 𝐯 for AOPT = 3. 
D1 D2 D3 
Components of vector 𝐝 for AOPT = 2.   
Remarks: 
The yield function is defined as 
where the equivalent stress 𝜎eq is defined as an anisotropic yield criterion 
𝑓 = 𝑓 ̅(σ) − [𝜎0 + 𝑅(𝜀𝑝)] 
𝜎eq = √𝐹(𝜎22 − 𝜎33)2 + 𝐺(𝜎33 − 𝜎11)2 + 𝐻(𝜎11 − 𝜎22)2 + 2𝐿𝜎23
2 + 2𝑀𝜎31
2  
2 + 2𝑁𝜎12
Where  F,  G,  H,  L,  M  and  N  are  constants  obtained  by  test  of  the  material  in  different 
orientations.  They are defined as 
𝐹 =
𝐺 =
𝐻 =
𝐿 =
𝑀 =
𝑁 =
(
(
(
2 +
𝑅22
2 +
𝑅33
2 +
𝑅11
2 −
𝑅33
2 −
𝑅11
2 −
𝑅22
2 ) 
𝑅11
2 ) 
𝑅22
2 ) 
𝑅33
2  
2𝑅23
2  
2𝑅31
2  
2𝑅12
The yield stress ratios are defined as follows 
𝑅11 =
𝑅22 =
𝑅33 =
𝑅12 =
𝑅23 =
𝑅31 =
𝜎̅̅̅̅̅11
𝜎0
𝜎̅̅̅̅̅22
𝜎0
𝜎̅̅̅̅̅33
𝜎0
𝜎̅̅̅̅̅12
𝜏0
𝜎̅̅̅̅̅23
𝜏0
𝜎̅̅̅̅̅31
𝜏0
where  𝜎𝑖𝑗  is  the  measured  yield  stress  values,  𝜎0  is  the  reference  yield  stress  and 
𝜏0 = 𝜎0/√3.  
The  strain  hardening  is  either  defined  by  the  load  curve  or  the  strain  hardening  R  is 
defined by the extended Voce law, 
𝑅(𝜀𝑝) = ∑ 𝑄𝑅𝑖[1 − exp(−𝐶𝑅𝑖𝜀𝑝)]
𝑖=1
where  𝜀𝑝  is  the  effective  (or  accumulated)  plastic  strain,  and  𝑄𝑅𝑖  and  𝐶𝑅𝑖  are  strain 
hardening parameters.
*MAT_JOHNSON_HOLMQUIST_CERAMICS 
This is Material Type 110.  This Johnson-Holmquist Plasticity Damage Model is useful 
for  modeling  ceramics,  glass  and  other  brittle  materials.    A  more  detailed  description 
can be found in a paper by Johnson and Holmquist [1993]. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
Variable 
EPSI 
Type 
F 
  Card 3 
Variable 
1 
D1 
Type 
F 
  VARIABLE   
MID 
2 
RO 
F 
2 
T 
F 
2 
D2 
F 
3 
G 
F 
3 
4 
A 
F 
4 
5 
B 
F 
5 
6 
C 
F 
6 
7 
M 
F 
7 
8 
N 
F 
8 
SFMAX 
HEL 
PHEL 
BETA 
F 
F 
F 
F 
3 
K1 
F 
4 
K2 
F 
5 
K3 
F 
6 
FS 
F 
DESCRIPTION
7 
8 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Density 
G 
A 
B 
C 
M 
Shear modulus 
Intact normalized strength parameter 
Fractured normalized strength parameter 
Strength parameter (for strain rate dependence) 
Fractured strength parameter (pressure exponent)
VARIABLE   
DESCRIPTION
N 
EPS0 
T 
SFMAX 
HEL 
PHEL 
BETA 
D1 
D2 
K1 
K2 
K3 
FS 
Intact strength parameter (pressure exponent). 
Quasi-static threshold strain rate.  See *MAT_015. 
Maximum tensile pressure strength. 
Maximum  normalized  fractured  strength  (defaults  to  1020  when 
set to 0.0). 
Hugoniot elastic limit. 
Pressure component at the Hugoniot elastic limit. 
Fraction  of  elastic  energy  loss  converted  to  hydrostatic  energy
(affects  bulking  pressure  (history  variable  1)  that  accompanies
damage). 
Parameter for plastic strain to fracture. 
Parameter for plastic strain to fracture (exponent). 
First pressure coefficient (equivalent to the bulk modulus). 
Second pressure coefficient. 
Third pressure coefficient. 
Element deletion criterion. 
FS.LT.0:  fail if 𝑝∗ + 𝑡∗ < 0 (tensile failure). 
FS.EQ.0:  no failure (default). 
FS.GT.0:  fail if  the effective plastic strain > FS. 
Remarks: 
The equivalent stress for a ceramic-type material is given by 
𝜎 ∗ = 𝜎𝑖
∗ − 𝐷(𝜎𝑖
∗ − 𝜎𝑓
∗) 
where 
∗ = 𝑎(𝑝∗ + 𝑡∗)𝑛(1 + 𝑐ln𝜀̇∗) 
𝜎𝑖
represents the intact, undamaged behavior.  The superscript, '*', indicates a normalized 
quantity.    The  stresses  are  normalized  by  the  equivalent  stress  at  the  Hugoniot  elastic 
limit, the pressures are normalized by the pressure at the Hugoniot elastic limit, and the
strain  rate  by  the  reference  strain  rate  defined  in  the  input.    In  this  equation  𝑎  is  the 
intact  normalized  strength  parameter,  𝑐  is  the  strength  parameter  for  strain  rate 
dependence, 𝜀̇∗ is the normalized plastic strain rate, and,  
𝑡∗ =
𝑝∗ =
PHEL
PHEL
,
,
where 𝑇 is the maximum tensile pressure strength, PHEL is the pressure component at 
the Hugoniot elastic limit, and p is the pressure. 
𝐷 = ∑
Δ𝜀𝑝
𝑝  
𝜀𝑓
represents  the  accumulated  damage  (history  variable  2)  based  upon  the  increase  in 
plastic strain per computational cycle and the plastic strain to fracture 
and 
𝑝 = 𝑑1(𝑝∗ + 𝑡∗)𝑑2 
𝜀𝑓
∗ = 𝑏(𝑝∗)𝑚(1 + 𝑐 ln𝜀̇) ≤ SFMAX 
𝜎𝑓
represents the damaged behavior.  The parameter d1 controls the rate at which damage 
accumulates.  If it is made 0, full damage occurs in one time step i.e.  instantaneously.  It 
is  also  the  best  parameter  to  vary  if  one  attempts  to  reproduce  results  generated  by 
another finite element program. 
In undamaged material, the hydrostatic pressure is given by 
in compression and 
𝑃 = 𝑘1𝜇 + 𝑘2𝜇2 + 𝑘3𝜇3 
𝑃 = 𝑘1𝜇 
⁄
in  tension  where  𝜇 = 𝜌 𝜌0 − 1
.    When  damage  starts  to  occur,  there  is  an  increase  in 
pressure.    A  fraction,  between  0  and  1,  of  the  elastic  energy  loss,  𝛽,  is  converted  into 
hydrostatic potential energy (pressure).  The details of this pressure increase are given 
in the reference. 
Given HEL and G, 𝜇hel can be found iteratively from 
2 + 𝑘3𝜇hel
and, subsequently, for normalization purposes, 
HEL = 𝑘1𝜇hel + 𝑘2𝜇hel
3 + (4 3⁄ )𝑔(𝜇hel/(1 + 𝜇hel) 
2-576 (EOS) 
LS-DYNA R10.0 
𝑃hel = 𝑘1𝜇hel + 𝑘2𝜇hel
and 
These are calculated automatically by LS-DYNA if 𝜌𝑓0 is zero on input.
𝜎hel = 1.5(hel − 𝑝hel)
*MAT_JOHNSON_HOLMQUIST_CONCRETE 
This  is  Material  Type  111.    This  model  can  be  used  for  concrete  subjected  to  large 
strains, high strain rates and high pressures.  The equivalent strength is expressed as a 
function  of  the  pressure,  strain  rate,  and  damage.    The  pressure  is  expressed  as  a 
function  of  the  volumetric  strain  and  includes  the  effect  of  permanent  crushing.    The 
damage is accumulated as a function of the plastic volumetric strain, equivalent plastic 
strain  and  pressure.    A  more  detailed  description  of  this  model  can  be  found  in  the 
paper by Holmquist, Johnson, and Cook [1993]. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
Variable 
Type 
  Card 3 
Variable 
1 
T 
F 
1 
D1 
Type 
F 
  VARIABLE   
MID 
2 
RO 
F 
2 
3 
G 
F 
3 
4 
A 
F 
4 
EPS0 
EFMIN 
SFMAX 
F 
F 
F 
2 
D2 
F 
3 
K1 
F 
4 
K2 
F 
5 
B 
F 
5 
PC 
F 
5 
K3 
F 
6 
C 
F 
6 
UC 
F 
6 
FS 
F 
7 
N 
F 
7 
PL 
F 
7 
8 
FC 
F 
8 
UL 
F 
8 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density. 
G 
A 
B 
Shear modulus. 
Normalized cohesive strength. 
Normalized pressure hardening.
VARIABLE   
DESCRIPTION
C 
N 
FC 
T 
Strain rate coefficient. 
Pressure hardening exponent. 
Quasi-static uniaxial compressive strength. 
Maximum tensile hydrostatic pressure. 
EPS0 
Quasi-static threshold strain rate.  See *MAT_015. 
EFMIN 
Amount of plastic strain before fracture. 
SFMAX 
Normalized maximum strength. 
PC 
UC 
PL 
UL 
D1 
D2 
K1 
K2 
K3 
FS 
Crushing pressure. 
Crushing volumetric strain. 
Locking pressure. 
Locking volumetric strain. 
Damage constant. 
Damage constant. 
Pressure constant. 
Pressure constant. 
Pressure constant. 
Failure type: 
FS.LT.0:  fail if damage strength < 0 
FS.EQ.0: fail if 𝑃∗ + 𝑇∗ ≤ 0  (tensile failure). 
FS.GT.0:  fail if  the effective plastic strain > FS. 
Remarks: 
The normalized equivalent stress is defined as 
𝑓′𝑐
𝜎 ∗ =
where  𝜎  is  the  actual  equivalent  stress,  and  𝑓′  is  the  quasi-static  uniaxial  compressive 
strength.  The expression is defined as: 
𝜎 ∗ = [𝐴(1 − 𝐷) + 𝐵𝑃∗𝑁][1 + 𝐶ln(𝜀̇∗)] 
where 𝐷 is the damage parameter, 𝑃∗ = 𝑃 𝑓′𝑐⁄  is the normalized pressure and 𝜀̇∗ = 𝜀̇ 𝜀̇0⁄  
is the dimensionless strain rate.  The model incrementally accumulates damage, D, both 
from equivalent plastic strain and plastic volumetric strain, and is expressed as 
𝐷 = ∑
Δ𝜀𝑝 + Δ𝜇𝑝
𝐷1(𝑃∗ + 𝑇∗)𝐷2
where Δ𝜀𝑝 and Δ𝜇𝑝 are the equivalent plastic strain and plastic volumetric strain, 𝐷1and 
𝐷2 are material constants and 𝑇∗ = 𝑇 𝑓c
′⁄  is the normalized maximum tensile hydrostatic 
pressure. 
The damage strength, DS, is defined in compression when 𝑃∗ > 0 as 
DS = 𝑓𝑐
′ min[SFMAX, 𝐴(1 − 𝐷) + 𝐵𝑃∗𝑁
] [1 + 𝐶 ∗ ln(𝜀̇∗)] 
or in tension if 𝑃∗ < 0, as 
DS = 𝑓𝑐
′ max [0, 𝐴(1 − 𝐷) − 𝐴 (
)] [1 + 𝐶 ∗ ln(𝜀̇∗)] 
𝑃∗
The pressure for fully dense material is expressed as 
𝑃 = 𝐾1𝜇̅̅̅̅ + 𝐾2𝜇̅̅̅̅2 + 𝐾3𝜇̅̅̅̅3 
where  𝐾1  ,  𝐾2  and  𝐾3  are  material  constants  and  the  modified  volumetric  strain  is 
defined as 
where 𝜇lock is the locking volumetric strain.
𝜇̅̅̅̅ =
𝜇 − 𝜇lock
1 + 𝜇lock
*MAT_FINITE_ELASTIC_STRAIN_PLASTICITY 
This  is  Material  Type  112.    An  elasto-plastic  material  with  an  arbitrary  stress  versus 
strain curve and arbitrary strain rate dependency can be defined.  The elastic response 
of  this  model  uses  a  finite  strain  formulation  so  that  large  elastic  strains  can  develop 
before  yielding  occurs.    This  model  is  available  for  solid  elements  only.    See  Remarks 
below. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
6 
7 
8 
SIGY 
ETAN 
F 
F 
Default 
none 
none 
none 
none 
none 
0.0 
  Card 2 
Variable 
Type 
Default 
1 
C 
F 
0 
  Card 3 
1 
2 
P 
F 
0 
2 
3 
4 
5 
6 
7 
8 
LCSS 
LCSR 
F 
0 
3 
F 
0 
4 
5 
6 
7 
8 
Variable 
EPS1 
EPS2 
EPS3 
EPS4 
EPS5 
EPS6 
EPS7 
EPS8 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ES1 
ES2 
ES3 
ES4 
ES5 
ES6 
ES7 
ES8 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
SIGY 
ETAN 
C 
P 
LCSS 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
Yield stress. 
Tangent modulus, ignored if (LCSS.GT.0) is defined. 
Strain rate parameter, C, see formula below. 
Strain rate parameter, P, see formula below. 
Load  curve  ID  or  Table  ID.    Load  curve  ID  defining  effective
stress  versus  effective  plastic  strain.    If  defined  EPS1  -  EPS8  and 
ES1  -  ES8  are  ignored.      The  table  ID  defines  for  each  strain  rate
value  a  load  curve  ID  giving  the  stress  versus  effective  plastic
strain for that rate, See Figure M24-1.  The stress versus effective 
plastic strain curve for the lowest value of strain rate is used if the
strain  rate  falls  below  the  minimum  value.    Likewise,  the  stress
versus effective plastic strain curve for the highest value of strain
rate  is  used  if  the  strain  rate  exceeds  the  maximum  value.    The
strain rate parameters: C and P; the curve ID, LCSR; EPS1 - EPS8 
and ES1 - ES8 are ignored if a Table ID is defined. 
LCSR 
Load curve ID defining strain rate scaling effect on yield stress.
VARIABLE   
EPS1 - EPS8 
DESCRIPTION
Effective  plastic  strain  values  (optional  if  SIGY  is  defined).    At
least  2  points  should  be  defined.    The  first  point  must  be  zero
corresponding  to  the  initial  yield  stress.    WARNING:  If  the  first
point is nonzero the yield stress is extrapolated to determine the
initial  yield.    If  this  option  is  used  SIGY  and  ETAN  are  ignored
and may be input as zero. 
ES1 - ES8 
Corresponding yield stress values to EPS1 - EPS8. 
Remarks: 
The  stress  strain  behavior  may  be  treated  by  a  bilinear  stress  strain  curve  by  defining 
the tangent modulus, ETAN.  Alternately, a curve similar to that shown in Figure M10-1 
is expected to be defined by (EPS1,ES1) - (EPS8,ES8); however, an effective stress versus 
effective plastic strain curve (LCSS) may be input instead if eight points are insufficient.  
The cost is roughly the same for either approach.  The most general approach is to use 
the table definition (LCSS) discussed below. 
Three options to account for strain rate effects are possible. 
1.  Strain rate may be accounted for using the Cowper and Symonds model which 
scales the yield stress with the factor 
1 + (
𝑝⁄
)
𝜀̇
where 𝜀̇ is the strain rate, 𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗. 
2.  For  complete  generality  a  load  curve  (LCSR)  to  scale  the  yield  stress  may  be 
input instead.  In this curve the scale factor versus strain rate is defined.   
3. 
If different stress versus strain curves can be provided for various strain rates, 
the  option  using  the  reference  to  a  table  (LCSS)  can  be  used.    Then  the  table 
input in *DEFINE_TABLE has to be used, see Figure M24-1.
*MAT_TRIP 
This  is  Material  Type 113.    This  isotropic  elasto-plastic  material  model  applies  to  shell 
elements only.  It features a special hardening law aimed at modelling the temperature 
dependent  hardening  behavior  of  austenitic  stainless  TRIP-steels.    TRIP  stands  for 
Transformation Induced Plasticity.  A detailed description of this material model can be 
found in Hänsel, Hora, and Reissner [1998] and Schedin, Prentzas, and Hilding [2004]. 
  Card  1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
Default 
  Card  2 
Variable 
Type 
Default 
1 
A 
F 
2 
B 
F 
  Card  3 
1 
2 
Variable 
AHS 
BHS 
3 
E 
F 
3 
C 
3 
M 
4 
PR 
5 
CP 
6 
T0 
7 
8 
TREF 
TA0 
4 
D 
4 
N 
5 
P 
6 
Q 
7 
8 
E0MART 
VM0 
5 
6 
EPS0 
HMART 
7 
K1 
8 
K2 
Type 
Default 
  VARIABLE   
MID 
DESCRIPTION
Material identification. A unique number or label not exceeding 8 
characters must be specified. 
RO 
Mass density.
E 
PR 
CP 
T0 
TREF 
TA0 
A 
B 
C 
D 
P 
Q 
*MAT_113 
DESCRIPTION
Young’s modulus. 
Poisson’s ratio. 
Adiabatic temperature calculation option: 
EQ.0.0: Adiabatic temperature calculation is disabled. 
GT.0.0:  CP  is  the  specific  heat  Cp.    Adiabatic  temperature
calculation is enabled.  
Initial  temperature  T0  of  the  material  if  adiabatic  temperature 
calculation is enabled. 
Reference  temperature  for  output  of  the  yield  stress  as  history
variable 1. 
Reference  temperature  TA0,  the  absolute  zero  for  the  used 
temperature scale, e.g.  -273.15 if the Celsius scale is used and 0.0 
if the Kelvin scale is used. 
Martensite rate equation parameter A, see equations below. 
Martensite rate equation parameter B, see equations below. 
Martensite rate equation parameter C, see equations below. 
Martensite rate equation parameter D, see equations below. 
Martensite rate equation parameter p, see equations below. 
Martensite rate equation parameter Q, see equations below. 
E0MART 
Martensite rate equation parameter E0(mart) , see equations below. 
VM0 
The  initial  volume  fraction  of  martensite  0.0 < Vm0 < 1.0  may  be 
initialised using two different methods: 
GT.0.0: Vm0 is set to VM0. 
LT.0.0:  Can  be  used  only  when  there  are  initial  plastic  strains 
εp  present,  e.g. 
  when  using  *INITIAL_STRESS_-
SHELL.    The  absolute  value  of  VM0  is  then  the  load
curve  ID  for  a  function  f  that  sets  𝑉𝑚0 = 𝑓 (𝜀𝑝).  The 
function  f  must  be  a  monotonically  nondecreasing
function of 𝜀𝑝.
DESCRIPTION
*MAT_TRIP 
AHS 
BHS 
M 
N 
Hardening law parameter AHS, see equations below. 
Hardening law parameter BHS, see equations below. 
Hardening law parameter m, see equations below. 
Hardening law parameter n, see equations below. 
EPS0 
Hardening law parameter ε0, see equations below. 
HMART 
Hardening law parameter ΔHγ→α’ , see equations below. 
Hardening law parameter K1, see equations below. 
Hardening law parameter K2, see equations below. 
K1 
K2 
Remarks: 
Here a short description is given of the TRIP-material model.  The material model uses 
the von Mises yield surface in combination with isotropic hardening.  The hardening is 
temperature  dependent  and  therefore  this  material  model  must  be  run  either  in  a 
coupled  thermo-mechanical  solution,  using  prescribed  temperatures  or  using  the 
adiabatic temperature calculation option.  Setting the parameter CP to the specific heat 
Cp  of  the  material  activates  the  adiabatic  temperature  calculation  that  calculates  the 
temperature rate from the equation 
𝜎𝑖𝑗𝐷𝑖𝑗
𝜌𝐶𝑝
, 
𝑇̇ = ∑
𝑖,𝑗
where 𝛔: 𝐃𝑝 (the numerator) is the plastically dissipated heat.  Using the Kelvin scale is 
recommended, even though other scales may be used without problems. 
The  hardening  behavior  is  described  by  the  following  equations.    The  Martensite  rate 
equation is 
∂𝑉𝑚
∂𝜀̅𝑝 =
⎧0
{{
⎨
{{
⎩
𝑝 (
𝑉𝑚
1 − 𝑉𝑚
𝑉𝑚
where 
)
𝐵+1
𝐵 [1 − tanh(C + D × 𝑇)]
𝜀 < 𝐸0(mart)
exp (
𝑇 − 𝑇𝐴0
) 𝜀̅𝑝 ≥ 𝐸0(mart)
𝜀̅𝑝 = effective plastic strain and 
𝑇 = temperature.
The martensite fraction is integrated from the above rate equation: 
𝑉𝑚 = ∫
∂𝑉𝑚
∂𝜀̅𝑝
𝑑𝜀̅𝑝. 
It  always  holds  that  0.0 < Vm < 1.0.    The  initial  martensite  content  is  Vm0  and  must  be 
greater than zero and less than 1.0.  Note that Vm0 is not used during a restart or when 
initializing the Vm history variable using *INITIAL_STRESS_SHELL. 
The yield stress σy is 
𝜎𝑦 = {𝐵𝐻𝑆 − (𝐵𝐻𝑆 − 𝐴𝐻𝑆)exp(−𝑚[𝜀̅𝑝 + 𝜀0]𝑛)}(𝐾1 + 𝐾2𝑇) + Δ𝐻𝛾→𝛼′𝑉𝑚. 
The parameters p and B should fulfill the following condition 
1 + 𝐵
< 𝑝 
if  not  fulfilled  then  the  martensite  rate  will  approach  infinity  as  𝑉𝑚  approaches  zero.  
Setting the parameter 𝜀0 larger than zero, typical range 0.001-0.02 is recommended.  A 
part  from  the  effective  true  strain  a  few  additional  history  variables  are  output,  see 
below. 
History variables that are output for post-processing: 
Variable 
Description 
1 
2 
3 
Yield  stress  of  material  at  temperature  TREF.    Useful  to  evaluate  the 
strength of the material after e.g., a simulated forming operation. 
Volume fraction martensite, Vm 
CP.EQ.0.0: Not used 
CP.GT.0.0: Temperature from adiabatic temperature calculation
*MAT_LAYERED_LINEAR_PLASTICITY 
This  is  Material  Type  114.    A  layered  elastoplastic  material  with  an  arbitrary  stress 
versus  strain  curve  and  an  arbitrary  strain  rate  dependency  can  be  defined.    This 
material  must  be  used  with  the  user  defined  integration  rules,  see  *INTEGRATION-
SHELL, for modeling laminated composite and sandwich shells where each layer can be 
represented by elastoplastic behavior with constitutive constants that vary from layer to 
layer.  Lamination theory is applied to correct for the assumption of a uniform constant 
shear  strain  through  the  thickness  of  the  shell.    Unless  this  correction  is  applied,  the 
stiffness of the shell can be grossly incorrect leading to poor results.  Generally, without 
the correction the results are too stiff.   This model is available for  shell elements only.  
Also, see Remarks below. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
6 
7 
8 
SIGY 
ETAN 
FAIL 
TDEL 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
0.0 
10.E+20 
  Card 2 
Variable 
Type 
Default 
1 
C 
F 
0 
  Card 3 
1 
2 
P 
F 
0 
2 
3 
4 
5 
6 
7 
LCSS 
LCSR 
F 
0 
3 
F 
0 
4 
5 
6 
7 
8 
Variable 
EPS1 
EPS2 
EPS3 
EPS4 
EPS5 
EPS6 
EPS7 
EPS8 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
2-588 (EOS) 
LS-DYNA R10.0
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ES1 
ES2 
ES3 
ES4 
ES5 
ES6 
ES7 
ES8 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
SIGY 
ETAN 
FAIL 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
Yield stress.  
Tangent modulus, ignored if (LCSS.GT.0) is defined. 
Failure flag. 
LT.0.0:  User defined failure subroutine, matusr_24 in dyn21.F, 
is called to determine failure 
EQ.0.0: Failure is not considered.  This option is recommended
if failure is not of interest since many calculations will
be saved. 
GT.0.0:  Plastic strain to failure.  When the plastic strain reaches
this value, the element is deleted from the calculation. 
TDEL 
Minimum time step size for automatic element deletion. 
C 
P 
Strain rate parameter, C, see formula below. 
Strain rate parameter, P, see formula below.
LCSS 
*MAT_LAYERED_LINEAR_PLASTICITY 
DESCRIPTION
Load  curve  ID  or  Table  ID.    Load  curve  ID  defining  effective
stress  versus  effective  plastic  strain.    If  defined  EPS1  -  EPS8  and 
ES1  -  ES8  are  ignored.      The  table  ID  defines  for  each  strain  rate
value  a  load  curve  ID  giving  the  stress  versus  effective  plastic 
strain for that rate, See Figure M24-1.  The stress versus effective 
plastic strain curve for the lowest value of strain rate is used if the
strain  rate  falls  below  the  minimum  value.    Likewise,  the  stress
versus effective plastic strain curve for the 
highest  value  of  strain  rate  is  used  if  the  strain  rate  exceeds  the 
maximum value.  The strain rate parameters: C and P; the curve
ID, LCSR; EPS1 - EPS8 and ES1 - ES8 are ignored if a Table ID is 
defined. 
LCSR 
Load curve ID defining strain rate scaling effect on yield stress. 
EPS1 - EPS8 
Effective  plastic  strain  values  (optional  if  SIGY  is  defined).    At
least  2  points  should  be  defined.    The  first  point  must  be  zero
corresponding  to  the  initial  yield  stress.    WARNING:  If  the  first
point is nonzero the yield stress is extrapolated to determine the
initial  yield.    If  this  option  is  used  SIGY  and  ETAN  are  ignored
and may be input as zero. 
ES1 - ES8 
Corresponding yield stress values to EPS1 - EPS8. 
Remarks: 
The  stress  strain  behavior  may  be  treated  by  a  bilinear  stress  strain  curve  by  defining 
the tangent modulus, ETAN.  Alternately, a curve similar to that shown in Figure M10-1 
is  expected  to  be  defined  by  (EPS1,  ES1)  -  (EPS8,  ES8);  however,  an  effective  stress 
versus  effective  plastic  strain  curve  (LCSS)  may  be  input  instead  if  eight  points  are 
insufficient.    The  cost  is  roughly  the  same  for  either  approach.    The  most  general 
approach is to use the table definition (LCSS) discussed below. 
Three options to account for strain rate effects are possible. 
1.  Strain rate may be accounted for using the Cowper and Symonds model which 
scales the yield stress with the factor 
1 + (
𝑝⁄
)
𝜀̇
where 𝜀̇ is the strain rate, 𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗.
2.  For  complete  generality  a  load  curve  (LCSR)  to  scale  the  yield  stress  may  be 
input instead.  In this curve the scale factor versus strain rate is defined.   
3. 
If different stress versus strain curves can be provided for various strain rates, 
the  option  using  the  reference  to  a  table  (LCSS)  can  be  used.    Then  the  table 
input in *DEFINE_TABLE has to be used, see Figure M24-1.
*MAT_UNIFIED_CREEP 
This is Material Type 115.  This is an elastic creep model for modeling creep behavior 
when plastic behavior is not considered. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
A 
F 
6 
N 
F 
7 
M 
F 
8 
Default 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
E 
PR 
A 
N 
M 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
Stress coefficient. 
Stress exponent. 
Time exponent. 
Remarks: 
The effective creep strain, 𝜀̅𝑐, given as: 
𝜀̅𝑐 = 𝐴𝜎̅̅̅̅̅ 𝑛𝑡 ̅𝑚 
where  A,  n,  and  m  are  constants  and  𝑡 ̅  is  the  effective  time.    The  effective  stress,  𝜎̅̅̅̅̅,  is 
defined as: 
𝜎̅̅̅̅̅ = √
𝜎𝑖𝑗𝜎𝑖𝑗 
The creep strain, therefore, is only a function of the deviatoric stresses.  The volumetric 
behavior  for  this  material  is  assumed  to  be  elastic.    By  varying  the  time  constant  m
primary  creep  (m < 1),  secondary  creep  (m = 1),  and  tertiary  creep  (m > 1)  can  be 
modeled.  This model is described by Whirley and Henshall [1992].
*MAT_UNIFIED_CREEP 
This  is  Material  Type  115_O.    This  is  an  orthotropic  elastic  creep  model  for  modeling 
creep behavior when plastic behavior is not considered.  This material is only available 
for solid elements, and is available for both explicit and implicit dynamics. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E1 
F 
4 
E2 
F 
5 
E3 
F 
6 
7 
8 
PR21 
PR31 
PR32 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
Variable 
G12 
G23 
G13 
Type 
F 
F 
F 
4 
A 
F 
5 
N 
F 
6 
M 
F 
7 
8 
Default 
none 
none 
none 
none 
none 
none 
  Card 3 
1 
2 
Variable 
AOPT 
MACF 
Type 
F 
F 
3 
XP 
F 
4 
YP 
F 
5 
ZP 
F 
6 
A1 
F 
7 
A2 
F 
8 
A3 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none
Card 4 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
7 
8 
Default 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
MID 
RO 
Ei 
PRij 
Gij 
A 
N 
M 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s moduli. 
Elastic Poisson’s ratios. 
Elastic shear moduli. 
Stress coefficient. 
Stress exponent. 
Time exponent.
AOPT 
*MAT_UNIFIED_CREEP 
DESCRIPTION
Material  axes  option  : 
EQ.0.0:  locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES. 
EQ.1.0:  locally orthotropic with material axes determined by a
point  in  space  and  the  global  location  of  the  element
center;  this  is  the  a-direction.    This  option  is  for  solid 
elements only. 
EQ.2.0:  globally orthotropic with material axes determined by 
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0:  locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the 
element normal. 
EQ.4.0:  locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector  v,  and
an originating point, p, which define the centerline ax-
is.  This option is for solid elements only. 
LT.0.0:  the absolute value of AOPT is a coordinate system ID 
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
MACF 
Material axes change flag for brick elements: 
EQ.1:  No change, default, 
EQ.2:  switch material axes a and b, 
EQ.3:  switch material axes a and c, 
EQ.4:  switch material axes b and c. 
XP, YP, ZP 
Define coordinates of point p for AOPT = 1 and 4. 
A1, A2, A3 
Define components of vector a for AOPT = 2. 
V1, V2, V3 
Define components of vector v for AOPT = 3 and 4.
VARIABLE   
DESCRIPTION
D1, D2, D3 
Define components of vector d for AOPT = 2. 
BETA 
Material  angle  in  degrees  for  AOPT =  3,  may  be  overridden  on 
the element card, see *ELEMENT_SHELL_BETA or *ELEMENT_-
SOLID_ORTHO. 
Remarks: 
The stress-strain relationship is based on an additive split of the strain,  
Here, the multiaxial creep strain is given by 
𝜺̇ = 𝜺̇𝑒 + 𝜺̇𝑐. 
and 𝜀̅𝑐 is the effective creep strain, 𝒔 the deviatoric stress 
𝜺̇𝑐 = 𝜀̅𝑐̇
2𝒔
3𝜎̅̅̅̅̅
, 
and 𝜎̅̅̅̅̅ the effective stress 
𝒔 = 𝝈 −
tr(𝝈)𝑰. 
𝜎̅̅̅̅̅ = √
𝒔: 𝒔. 
The effective creep strain is given by 
where A, N, and M are constants. 
The stress increment is given by 
𝜀̅𝑐̇ = 𝐴𝜎̅̅̅̅̅ 𝑁𝑡𝑀, 
∆𝝈 = 𝑪∆𝜺𝑒 = 𝑪(∆𝜺 − ∆𝜺𝑐), 
where the constitutive matrix 𝑪 is taken as orthotropic and can be represented in Voigt 
notation by its inverse as
𝑪−1 =
𝐸1
𝜐12
𝐸1
𝜐13
𝐸1
−
−
𝜐21
𝐸2
𝐸2
𝜐23
𝐸2
−
−
𝜐31
𝐸3
𝜐32
𝐸3
𝐸3
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
.
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
𝐺13⎦
𝐺12
𝐺23
−
−
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
*MAT_116 
This  is  Material  Type  116.    This  material  is  for  modeling  the  elastic  responses  of 
composite  layups  that  have  an  arbitrary  number  of  layers  through  the  shell  thickness.  
A  pre-integration  is  used  to  compute  the  extensional,  bending,  and  coupling  stiffness 
for  use  with  the  Belytschko-Tsay  resultant  shell  formulation.    The  angles  of  the  local 
material  axes  are  specified  from  layer  to  layer  in  the  *SECTION_SHELL  input.    This 
material model must be used with the user defined integration rule for shells, see *IN-
TEGRATION_SHELL,  which  allows  the  elastic  constants  to  change  from  integration 
point  to  integration  point.    Since  the  stresses  are  not  computed  in  the  resultant 
formulation,  the  stresses  output  to  the  binary  databases  for  the  resultant  elements  are 
zero.  Note that this shell does not use laminated shell theory and that storage is allocated 
for just one integration point (as reported in D3HSP) regardless of the layers defined in 
the integration rule. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
EA 
F 
3 
4 
EB 
F 
4 
Variable 
GAB 
GBC 
GCA 
AOPT 
Type 
F 
F 
F 
F 
  Card 3 
Variable 
1 
XP 
Type 
F 
  Card 4 
Variable 
1 
V1 
Type 
F 
LS-DYNA R10.0 
2 
YP 
F 
2 
V2 
F 
3 
ZP 
F 
3 
V3 
F 
4 
A1 
F 
4 
D1 
F 
5 
EC 
F 
5 
5 
A2 
F 
5 
D2 
F 
6 
7 
8 
PRBA 
PRCA 
PRCB 
F 
6 
6 
A3 
F 
6 
D3 
F 
F 
7 
F 
8 
7 
8 
7 
8 
BETA
VARIABLE   
DESCRIPTION
MID 
RO 
EA 
EB 
EC 
PRBA 
PRCA 
PRCB 
GAB 
GBC 
GCA 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Ea, Young’s modulus in a-direction. 
Eb, Young’s modulus in b-direction. 
Ec, Young’s modulus in c-direction. 
ba, Poisson’s ratio ba. 
ca, Poisson’s ratio ca. 
cb, Poisson’s ratio cb. 
Gab, shear modulus ab. 
Gbc, shear modulus bc. 
Gca, shear modulus ca.
VARIABLE   
DESCRIPTION
AOPT 
Material axes option, see Figure M2-1: 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element  nodes  as  shown  in  Figure  M2-1.    Nodes  1,  2, 
and 4 of an element are identical to the nodes used for
the definition of a coordinate system as by *DEFINE_-
COORDINATE_NODES,  and  then  rotated  about  the 
shell element normal by an angle BETA. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the
element normal. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID 
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
XP, YP, ZP 
Define coordinates of point p for AOPT = 1 and 4. 
A1, A2, A3 
Define components of vector a for AOPT = 2. 
V1, V2, V3 
Define components of vector v for AOPT = 3 and 4. 
D1, D2, D3 
Define components of vector d for AOPT = 2. 
BETA 
Material angle in degrees for AOPT = 0 and 3, may be overridden 
on the element card, see *ELEMENT_SHELL_BETA. 
Remarks: 
This material law is based on standard composite lay-up theory.  The implementation, 
[Jones  1975],  allows  the  calculation  of  the  force,  N,  and  moment,  M,  stress  resultants 
from:  
⎧Nx
⎫
}
{
Ny
⎬
⎨
}
{
Nxy⎭
⎩
=
𝐴11 𝐴12 𝐴16
⎤
⎡
𝐴21 𝐴22 𝐴26
⎥
⎢
𝐴16 𝐴26 𝐴66⎦
⎣
}}⎫
{{⎧𝜀𝑥
𝜀𝑦
}}⎬
{{⎨
0⎭
𝜀𝑧
⎩
+
𝐵11 𝐵12 𝐵16
⎤
⎡
𝐵21 𝐵22 𝐵26
⎥
⎢
𝐵16 𝐵26 𝐵66⎦
⎣
{⎧𝜅x
}⎫
𝜅y
𝜅z⎭}⎬
⎩{⎨
⎧ 𝑀𝑥
⎫
}
{
My
⎬
⎨
}
{
Mxy⎭
⎩
=
𝐵11 𝐵12 𝐵16
⎤
⎡
𝐵21 𝐵22 𝐵26
⎥
⎢
𝐵16 𝐵26 𝐵66⎦
⎣
}}⎫
{{⎧𝜀𝑥
𝜀𝑦
}}⎬
{{⎨
0⎭
𝜀𝑧
⎩
+
𝐷11 𝐷12 𝐷16
⎤
𝐷21 𝐷22 𝐷26
⎥
𝐷16 𝐷26 𝐷66⎦
⎡
⎢
⎣
{⎧𝜅x
}⎫
𝜅y
𝜅z⎭}⎬
⎩{⎨
where 𝐴𝑖𝑗 is the extensional stiffness, 𝐷𝑖𝑗is the bending stiffness, and 𝐵𝑖𝑗 is the coupling 
stiffness  which  is  a  null  matrix  for  symmetric  lay-ups.    The  mid-surface  stains  and 
0   and  𝜅𝑖𝑗respectively.    Since  these  stiffness  matrices  are 
curvatures  are  denoted  by  𝜀𝑖𝑗
symmetric,  18  terms  are  needed  per  shell  element  in  addition  to  the  shell  resultants 
which are integrated in time.  This is considerably less storage than would typically be 
required with through thickness integration which requires a minimum of eight history 
variables  per  integration  point,  e.g.,  if  100  layers  are  used  800  history  variables  would 
be stored.  Not only is memory much less for this model, but the CPU time required is 
also considerably reduced.
*MAT_117 
This  is  Material  Type  117.    This  material  is  used  for  modeling  the  elastic  responses  of 
composites  where  a  pre-integration  is  used  to  compute  the  extensional,  bending,  and 
coupling  stiffness  coefficients  for  use  with  the  Belytschko-Tsay  resultant  shell 
formulation.    Since  the  stresses  are  not  computed  in  the  resultant  formulation,  the 
stresses output to the binary databases for the resultant elements are zero. 
NOTE: This material does not support specification of a ma-
terial  angle,  𝛽𝑖,  for  each  through-thickness  integra-
tion point of a shell. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
4 
5 
6 
7 
8 
3 
4 
5 
6 
7 
8 
Variable 
C11 
C12 
C22 
C13 
C23 
C33 
C14 
C24 
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
C34 
C44 
C15 
C25 
C35 
C45 
C55 
C16 
Type 
F 
  Card 4 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
C26 
C36 
C46 
C56 
C66 
AOPT 
Type 
F 
F 
F 
F 
F
Variable 
1 
XP 
Type 
F 
  Card 6 
Variable 
1 
V1 
Type 
F 
*MAT_COMPOSITE_MATRIX 
2 
YP 
F 
2 
V2 
F 
3 
ZP 
F 
3 
V3 
F 
4 
A1 
F 
4 
D1 
F 
5 
A2 
F 
5 
D2 
F 
6 
A3 
F 
6 
D3 
F 
7 
8 
7 
8 
BETA 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
CIJ 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
𝐶𝑖𝑗  coefficients  of  stiffness  matrix  in  the  material  coordinate
system. 
AOPT 
Material axes option, see Figure M2-1: 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element  nodes  as  shown  in  Figure  M2-1.    Nodes  1,  2, 
and 4 of an element are identical to the nodes used for 
the definition of a coordinate system as by *DEFINE_-
COORDINATE_NODES,  and  then  rotated  about  the 
shell element normal by an angle BETA. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  𝐯  with  the 
element normal. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
VARIABLE   
DESCRIPTION
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
XP, YP, ZP 
Define coordinates of point 𝐩 for AOPT = 1 and 4. 
A1, A2, A3 
Define components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
Define components of vector 𝐯 for AOPT = 3 and 4. 
D1, D2, D3 
Define components of vector 𝐝 for AOPT = 2. 
BETA 
Μaterial angle in degrees for AOPT = 0 and 3, may be overridden 
on the element card, see *ELEMENT_SHELL_BETA. 
Remarks: 
The calculation of the force, 𝑁𝑖𝑗, and moment, 𝑀𝑖𝑗, stress resultants is given in terms of 
the membrane strains, 𝜀𝑖
0, and shell curvatures 𝐶𝑖𝑗, 𝜅𝑖, as: 
𝑁𝑥
⎤
⎡
𝑁𝑦
⎥
⎢
⎥
⎢
𝑁𝑥𝑦
⎥
⎢
⎥
⎢
𝑀𝑥
⎥
⎢
⎥
⎢
𝑀𝑦
⎥
⎢
𝑀𝑥𝑦⎦
⎣
=
𝐶11 𝐶12 𝐶13 𝐶14 𝐶15 𝐶16
⎤
⎡
𝐶21 𝐶22 𝐶23 𝐶24 𝐶25 𝐶26
⎥
⎢
⎥
⎢
𝐶31 𝐶32 𝐶33 𝐶34 𝐶35 𝐶36
⎥
⎢
⎥
⎢
𝐶41 𝐶42 𝐶43 𝐶44 𝐶45 𝐶46
⎥
⎢
𝐶51 𝐶52 𝐶53 𝐶54 𝐶55 𝐶56
⎥
⎢
𝐶61 𝐶62 𝐶63 𝐶64 𝐶65 𝐶66⎦
⎣
𝜀𝑥
⎤
⎡
𝜀𝑦
⎥
⎢
⎥
⎢
⎥
⎢
𝜀𝑧
⎥
⎢
κ𝑥
⎥
⎢
𝜅𝑦
⎥
⎢
κ𝑧⎦
⎣
where  𝐶𝑖𝑗 = 𝐶𝑗𝑖.    In  this  model  this  symmetric  matrix  is  transformed  into  the  element 
local system and the coefficients are stored as element history variables.  In model type 
*MAT_COMPOSITE_DIRECT below, the resultants are already assumed to be given in 
the  element  local  system  which  reduces  the  storage  since  the  21  coefficients  are  not 
stored as history variables as part of the element data. 
The shell thickness is built into the coefficient matrix and, consequently, within the part 
ID, which references this material ID, the thickness must be uniform.
*MAT_COMPOSITE_DIRECT 
This  is  Material  Type  118.    This  material  is  used  for  modeling  the  elastic  responses  of 
composites  where  a  pre-integration  is  used  to  compute  the  extensional,  bending,  and 
coupling  stiffness  coefficients  for  use  with  the  Belytschko-Tsay  resultant  shell 
formulation.    Since  the  stresses  are  not  computed  in  the  resultant  formulation,  the 
stresses output to the binary databases for the resultant elements are zero. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
4 
5 
6 
7 
8 
3 
4 
5 
6 
7 
8 
Variable 
C11 
C12 
C22 
C13 
C23 
C33 
C14 
C24 
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
C34 
C44 
C15 
C25 
C35 
C45 
C55 
C16 
Type 
F 
  Card 4 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
C26 
C36 
C46 
C56 
C66 
Type 
F 
F 
F 
F 
F 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density.
VARIABLE   
DESCRIPTION
CIJ 
𝐶𝑖𝑗coefficients of the stiffness matrix. 
Remarks: 
The calculation of the force, 𝑁𝑖𝑗, and moment, 𝑀𝑖𝑗, stress resultants is given in terms of 
the membrane strains, 𝜀𝑖
⎫
0, and shell curvatures, 𝜅𝑖, as:  
⎧𝑁𝑥
𝑁𝑦
𝑁𝑥𝑦
𝑀𝑥
𝑀𝑦
𝑀𝑥𝑦⎭
𝐶11 𝐶12 𝐶13 𝐶14 𝐶15 𝐶16
⎤
⎡
𝐶21 𝐶22 𝐶23 𝐶24 𝐶25 𝐶26
⎥
⎢
⎥
⎢
𝐶31 𝐶32 𝐶33 𝐶34 𝐶35 𝐶36
⎥
⎢
⎥
⎢
𝐶41 𝐶42 𝐶43 𝐶44 𝐶45 𝐶46
⎥
⎢
𝐶51 𝐶52 𝐶53 𝐶54 𝐶55 𝐶56
⎥
⎢
𝐶61 𝐶62 𝐶63 𝐶64 𝐶65 𝐶66⎦
⎣
{{{{{
{{{{{
}}}}}
}}}}}
=
⎬
⎨
⎩
⎫
⎧𝜀𝑥
𝜀𝑦
𝜀𝑧
𝜅𝑥
𝜅𝑦
𝜅𝑥𝑦⎭
}}}}}
}}}}}
{{{{{
{{{{{
⎩
⎨
⎬
where 𝐶𝑖𝑗 = 𝐶𝑗𝑖.  In this model the stiffness coefficients are already assumed to be given 
in  the  element  local  system  which  reduces  the  storage.    Great  care  in  the  element 
orientation and choice of the local element system, see *CONTROL_ACCURACY, must 
be observed if this model is used. 
The shell thickness is built into the coefficient matrix and, consequently, within the part 
ID, which references this material ID, the thickness must be uniform.
*MAT_GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM 
This is Material Type 119.  This is a very general spring and damper model.  This beam 
  Additional 
the  MAT_SPRING_GENERAL_NONLINEAR  option. 
is  based  on 
unloading  options  have  been  included.    The  two  nodes  defining  the  beam  may  be 
coincident to give a zero length beam, or offset to give a finite length beam.  For finite 
length  discrete  beams  the  absolute  value  of  the  variable  SCOOR  in  the  SECTION_-
BEAM input should be set to a value of 2.0 or 3.0 to give physically correct behavior.   A 
triad is used to orient the beam for the directional springs. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
KT 
F 
3 
4 
KR 
F 
4 
5 
6 
7 
8 
IUNLD 
OFFSET 
DAMPF 
IFLAG 
I 
5 
F 
6 
F 
7 
I 
8 
Variable 
LCIDTR 
LCIDTS 
LCIDTT 
LCIDRR 
LCIDRS 
LCIDRT 
Type 
I 
  Card 3 
1 
I 
2 
I 
3 
I 
4 
I 
5 
I 
6 
7 
8 
Variable 
LCIDTUR  LCIDTUS  LCIDTUT  LCIDRUR  LCIDRUS  LCIDRUT 
Type 
I 
  Card 4 
1 
I 
2 
I 
3 
I 
4 
I 
5 
I 
6 
7 
8 
Variable 
LCIDTDR  LCIDTDS  LCIDTDT  LCIDRDR  LCIDRDS  LCIDRDT 
Type 
I 
I 
I 
I 
I
Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCIDTER 
LCIDTES 
LCIDTET 
LCIDRER  LCIDRES  LCIDRET 
Type 
I 
  Card 6 
1 
I 
2 
I 
3 
I 
4 
I 
5 
I 
6 
7 
8 
Variable 
UTFAILR  UTFAILS  UTFAILT  WTFAILR  WTFAILS  WTFAILT 
Type 
F 
  Card 7 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
7 
8 
Variable 
UCFAILR  UCFAILS  UCFAILT  WCFAILR WCFAILS WCFAILT 
Type 
F 
  Card 8 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
7 
8 
Variable 
IUR 
IUS 
IUT 
IWR 
IWS 
IWT 
Type 
F 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
KT 
KR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density, see also volume in *SECTION_BEAM definition. 
Translational stiffness for unloading option 2.0. 
Rotational stiffness for unloading option 2.0.
DAMPF 
IFLAG 
*MAT_GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM 
DESCRIPTION
Damping factor for stability.  Values in the neighborhood of unity
are  recommended.    This  damping  factor  is  properly  scaled  to
eliminate time step size dependency.  Also, it is active if and only
if the local stiffness is defined. 
Flag for switching between the displacement (default IFLAG = 0) 
and  linear  strain  (IFLAG = 1)  formulations.    The  displacement 
formulation  is  the  one  used  in  all  other  models.    For  the  linear
strain  formulation,  the  displacements  and  velocities  are  divided
by the initial length of the beam. 
IUNLD 
Unloading option (Also see Figure M119-1.): 
EQ.0.0: Loading and unloading follow loading curve 
EQ.1.0: Loading  follows  loading  curve,  unloading  follows
unloading curve.  The unloading curve ID if undefined
is taken as the loading curve. 
EQ.2.0: Loading  follows  loading  curve,  unloading  follows
unloading stiffness, KT or KR, to the unloading curve.
The  loading  and  unloading  curves  may  only  intersect
at the origin of the axes. 
EQ.3.0: Quadratic unloading from peak displacement value to
a permanent offset. 
OFFSET 
LCIDTR 
if 
the 
Offset factor between 0 and 1.0 to determine permanent set upon
in 
unloading 
compression  and  tension  are  equal  to  the  product  of  this  offset 
value  and  the  maximum  compressive  and  tensile  displacements,
respectively. 
  The  permanent  sets 
IUNLD = 3.0. 
Load curve ID defining translational force resultant along local r-
axis  versus  relative  translational  displacement.    If  zero,  no
stiffness  related  forces  are  generated  for  this  degree  of  freedom.
The  loading  curves  must  be  defined  from  the  most  negative
displacement  to  the  most  positive  displacement.    The  force  does
not need to increase monotonically.  The curves in this input are
linearly  extrapolated  when  the  displacement  range  falls  outside
the curve definition. 
LCIDTS 
Load curve ID defining translational force resultant along local s-
axis versus relative translational displacement.
VARIABLE   
LCIDTT 
LCIDRR 
LCIDRS 
LCIDRT 
LCIDTUR 
DESCRIPTION
Load curve ID defining translational force resultant along local t-
axis versus relative translational displacement. 
Load curve ID defining rotational moment resultant about local r-
axis versus relative rotational displacement. 
Load curve ID defining rotational moment resultant about local s-
axis versus relative rotational displacement. 
Load curve ID defining rotational moment resultant about local t-
axis versus relative rotational displacement. 
this  curve  must 
force  values  defined  by 
Load curve ID defining translational force resultant along local r-
axis versus relative translational displacement during unloading.
The 
increase
monotonically  from  the  most  negative  displacement  to  the  most
positive  displacement.    For  IUNLD = 1.0,  the  slope  of  this  curve 
must equal or exceed the loading curve for stability reasons.  This
is  not  the  case  for  IUNLD = 2.0.      For  loading  and  unloading  to 
follow  the  same  path  simply  set  LCIDTUR = LCIDTR.    For  options 
IUNLD = 0.0  or  3.0  the  unloading  curve  is  not  required.    For 
IUNLD = 2.0,  if  LCIDTUR  is  left  blank  or  zero,  the  default  is  to
use the same curve for unloading as for loading. 
LCIDTUS 
LCIDTUT 
LCIDRUR 
LCIDRUS 
LCIDRUT 
LCIDTDR 
LCIDTDS 
Load curve ID defining translational force resultant along local s-
axis versus relative translational displacement during unloading.
Load curve ID defining translational force resultant along local t-
axis versus relative translational displacement during unloading.
Load curve ID defining rotational moment resultant about local r-
axis versus relative rotational displacement during unloading. 
Load curve ID defining rotational moment resultant about local s-
axis versus relative rotational displacement during unloading. 
Load curve ID defining rotational moment resultant about local t-
axis versus relative rotational displacement during unloading.  If 
zero, no viscous forces are generated for this degree of freedom.   
Load  curve  ID  defining  translational  damping  force  resultant
along local r-axis versus relative translational velocity. 
Load  curve  ID  defining  translational  damping  force  resultant 
along local s-axis versus relative translational velocity.
LCIDTDT 
LCIDRDR 
LCIDRDS 
LCIDRDT 
LCIDTER 
LCIDTES 
LCIDTET 
LCIDRER 
LCIDRES 
LCIDRET 
UTFAILR 
UTFAILS 
UTFAILT 
WTFAILR 
*MAT_GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM 
DESCRIPTION
Load  curve  ID  defining  translational  damping  force  resultant
along local t-axis versus relative translational velocity. 
Load  curve  ID  defining  rotational  damping  moment  resultant
about local r-axis versus relative rotational velocity. 
Load  curve  ID  defining  rotational  damping  moment  resultant
about local s-axis versus relative rotational velocity. 
Load  curve  ID  defining  rotational  damping  moment  resultant 
about local t-axis versus relative rotational velocity. 
Load  curve  ID  defining  translational  damping  force  scale  factor
versus relative displacement in local r-direction. 
Load  curve  ID  defining  translational  damping  force  scale  factor 
versus relative displacement in local s-direction. 
Load  curve  ID  defining  translational  damping  force  scale  factor
versus relative displacement in local t-direction. 
Load  curve  ID  defining  rotational  damping  moment  resultant 
scale factor versus relative displacement in local r-rotation. 
Load  curve  ID  defining  rotational  damping  moment  resultant
scale factor versus relative displacement in local s-rotation. 
Load  curve  ID  defining  rotational  damping  moment  resultant 
scale factor versus relative displacement in local t-rotation. 
Optional, translational displacement at failure in tension.  If zero,
the  corresponding  displacement,  ur,  is  not  considered  in  the 
failure calculation. 
Optional, translational displacement at failure in tension.  If zero,
the  corresponding  displacement,  us,  is  not  considered  in  the 
failure calculation. 
Optional, translational displacement at failure in tension.  If zero,
the  corresponding  displacement,  ut,  is  not  considered  in  the 
failure calculation. 
Optional, rotational displacement at failure in tension.  If zero, the
corresponding  rotation,  θr,  is  not  considered  in  the  failure 
calculation.
VARIABLE   
WTFAILS 
WTFAILT 
UCFAILR 
UCFAILS 
UCFAILT 
WCFAILR 
WCFAILS 
WCFAILT 
IUR 
IUS 
IUT 
IWR 
IWS 
IWT 
DESCRIPTION
Optional, rotational displacement at failure in tension.  If zero, the 
corresponding  rotation,  θs,  is  not  considered  in  the  failure 
calculation. 
Optional  rotational displacement at failure in tension.  If zero, the
corresponding  rotation,  θt,  is  not  considered  in  the  failure 
calculation. 
Optional, translational displacement at failure in compression.  If
zero, the corresponding displacement, ur, is not considered in the 
failure calculation.  Define as a positive number. 
Optional, translational displacement at failure in compression.  If
zero, the corresponding displacement, us, is not considered in the 
failure calculation.  Define as a positive number. 
Optional, translational displacement at failure in compression.  If 
zero, the corresponding displacement, ut, is not considered in the 
failure calculation.  Define as a positive number. 
Optional,  rotational  displacement  at  failure  in  compression.    If
zero,  the  corresponding  rotation,  θr,  is  not  considered  in  the 
failure calculation.  Define as a positive number. 
Optional,  rotational  displacement  at  failure  in  compression.    If
zero,  the  corresponding  rotation,  θs,  is  not  considered  in  the 
failure calculation.  Define as a positive number. 
Optional,  rotational  displacement  at  failure  in  compression.    If
zero,  the  corresponding  rotation,  θt,  is  not  considered  in  the 
failure calculation.  Define as a positive number. 
Initial translational displacement along local r-axis. 
Initial translational displacement along local s-axis. 
Initial translational displacement along local t-axis. 
Initial rotational displacement about the local r-axis. 
Initial rotational displacement about the local s-axis. 
Initial rotational displacement about the local t-axis.
*MAT_GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM 
Catastrophic  failure,  which  is  based  on  displacement  resultants,  occurs  if  either  of  the 
following inequalities are satisfied: 
)
(
𝑢𝑟
tfail
𝑢𝑟
+ (
𝑢𝑠
tfail
𝑢𝑠
)
+ (
𝑢𝑡
tfail
𝑢𝑡
)
+ (
𝜃𝑟
tfail
𝜃𝑟
)
+ (
)
+
𝜃𝑠
tfail
𝜃𝑠
⎜⎛ 𝜃𝑡
𝑡𝑓𝑎𝑖𝑙
𝜃𝑡
⎝
⎟⎞
⎠
(
𝑢𝑟
cfail
𝑢𝑟
)
+ (
𝑢𝑠
cfail
𝑢𝑠
)
+ (
𝑢𝑡
cfail
𝑢𝑡
)
+ (
𝜃𝑟
cfail
𝜃𝑟
)
+ (
𝜃𝑠
cfail
𝜃𝑠
)
+ (
𝜃𝑡
cfail
𝜃𝑡
− 1. ≥ 0 
)
− 1. ≥ 0 
After  failure  the  discrete  element  is  deleted.    If  failure  is  included  either  the  tension 
failure or the compression failure or both may be used. 
Unload = 0
Loading-unloading
curve
Unload = 2
Unloading
curve
DISPLACEMENT
Unloading
curve
DISPLACEMENT
Unload = 1
Unload = 3
DISPLACEMENT
umin
× OFFSET
umin
Quadratic
unloading
DISPLACEMENT
Figure M119-1.  Load and unloading behavior.
There  are  two  formulations  for  calculating  the  force.    The  first  is  the  standard 
displacement formulation, where, for example, the force in a linear spring is 
𝐹 = −𝐾Δℓ 
for a change in length of the beam of Δℓ.  The second formulation is based on the linear 
strain, giving a force of 
𝐹 = −𝐾
Δℓ
ℓ0
for a beam with an initial length of  ℓ0.  This option is useful when there are springs of 
different  lengths  but  otherwise  similar  construction  since  it  automatically  reduces  the 
stiffness of the spring as the length increases, allowing an entire family of springs to be 
modeled  with  a  single  material.    Note  that  all  the  displacement  and  velocity 
components  are  divided  by  the  initial  length,  and  therefore  the  scaling  applies  to  the 
damping and rotational stiffness.
*MAT_GURSON 
This is Material Type 120.  This is the Gurson dilatational-plastic model.  This model is 
available  for  shell  and  solid  elements.    A  detailed  description  of  this  model  can  be 
found in the following references: Gurson [1975, 1977], Chu and Needleman [1980] and 
Tvergaard  and  Needleman  [1984].    The  implementation  in  LS-DYNA  is  based  on  the 
implementation  of  Feucht  [1998]  and  Faßnacht  [1999],  which  was  recoded  at  LSTC.   
Strain rate dependency can be defined via a Table definition. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
SIGY 
F 
6 
N 
F 
7 
Q1 
F 
8 
Q2 
F 
Default 
none 
none 
none 
none 
none 
0.0 
none 
none 
  Card 2 
Variable 
Type 
Default 
1 
FC 
F 
0 
  Card 3 
1 
2 
F0 
F 
0 
2 
3 
EN 
F 
0 
3 
4 
SN 
F 
0 
4 
5 
FN 
F 
0 
5 
6 
7 
8 
ETAN 
ATYP 
FF0 
F 
0 
6 
F 
0 
7 
F 
0 
8 
Variable 
EPS1 
EPS2 
EPS3 
EPS4 
EPS5 
EPS6 
EPS7 
EPS8 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ES1 
ES2 
ES3 
ES4 
ES5 
ES6 
ES7 
ES8 
Type 
Default 
  Card 5 
Variable 
Type 
Default 
F 
0 
1 
L1 
F 
0 
  Card 6 
1 
F 
0 
2 
L2 
F 
0 
2 
F 
0 
3 
L3 
F 
0 
3 
F 
0 
4 
L4 
F 
0 
4 
F 
0 
5 
F 
0 
6 
F 
0 
7 
F 
0 
8 
FF1 
FF2 
FF3 
FF4 
F 
0 
5 
F 
0 
6 
F 
0 
7 
F 
0 
8 
Variable 
LCSS 
LCLF 
NUMINT 
LCF0 
LCFC 
LCFN 
VGTYP 
DEXP 
Type 
Default 
F 
0 
F 
0 
F 
1.0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
3.0 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
SIGY 
N 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
Yield stress. 
Exponent for Power law.  This value is only used if ATYP = 1 and 
LCSS = 0.
Q1 
Q2 
FC 
F0 
EN 
*MAT_GURSON 
DESCRIPTION
Gurson flow function parameter 𝑞1. 
Gurson flow function parameter 𝑞2. 
Critical  void  volume  fraction  𝑓𝑐  where  voids  begin  to  aggregate. 
This value is only used if LCFC = 0. 
Initial void volume fraction 𝑓0. This value is only used if LCF0 = 0.
Mean nucleation strain 𝜀𝑁. 
GT.0.0:  Constant value, 
LT.0.0:  Load  curve  ID = (-EN)  which  defines  mean  nucleation 
strain 𝜀𝑁  as a function of element length. 
SN 
Standard deviation 𝑠𝑁 of the normal distribution of 𝜀𝑁.  
GT.0.0:  Constant value, 
LT.0.0:  Load  curve 
ID = (-SN)  which  defines  standard 
deviation 𝑠𝑁 of the normal distribution of 𝜀𝑁 as a func-
tion of element length. 
FN 
ETAN 
Void volume fraction of nucleating particles 𝑓𝑁. This value is only 
used if LCFN = 0. 
Hardening  modulus.    This  value  is  only  used  if  ATYP = 2  and 
LCSS = 0. 
ATYP 
Type of hardening. 
EQ.0.0: Ideal plastic, 
EQ.1.0: Power law, 
𝜎𝑌 = SIGY. 
𝜎𝑌 = SIGY × (
𝜀𝑝 + SIGY/E
SIGY/E
1/N
)
EQ.2.0: Linear hardening, 
𝜎𝑌 = SIGY +
E × ETAN
E − ETAN
𝜀𝑝. 
EQ.3.0: 8 points curve. 
FF0 
Failure  void  volume  fraction  𝑓𝐹.  This  value  is  only  used  if  no 
curve is given by (L1, FF1) – (L4, FF4) and LCFF = 0.
EPS1 - EPS8 
*MAT_120 
DESCRIPTION
Effective  plastic  strain  values.    The  first  point  must  be  zero 
corresponding to the initial yield stress.  At least 2 points should
be defined.  These values are used if ATYP = 3 and LCSS = 0. 
ES1 - ES8 
Corresponding yield stress values to EPS1 – EPS8.  These values 
are used if ATYP = 3 and LCSS = 0. 
L1 - L4 
Element length values.  These values are only used if LCFF = 0 
FF1 - FF4 
LCSS 
LCFF 
NUMINT 
Corresponding  failure  void  volume  fraction.    These  values  are
only used if LCFF = 0. 
Load  curve  ID  or  Table  ID.    ATYP  is  ignored  with  this  option.
Load  curve  ID  defining  effective  stress  versus  effective  plastic
strain.  Table ID defines for each strain rate value a load curve ID
giving  the  effective  stress  versus  effective  plastic  strain  for  that 
rate .   The stress-strain curve for the lowest value 
of  strain  rate  is  used  if  the  strain  rate  falls  below  the  minimum
value.    Likewise,  the  stress-strain  curve  for  the  highest  value  of 
strain rate is used if the strain rate exceeds the maximum value. 
NOTE: The strain rate values defined in the table may be given as
the  natural  logarithm  of  the  strain  rate.    If  the  first  stress-strain 
curve in the table corresponds to a negative strain rate, LS-DYNA 
assumes that the natural logarithm of the strain rate value is used. 
Since  the  tables  are  internally  discretized  to  equally  space  the
points,  natural  logarithms  are  necessary,  for  example,  if  the
curves correspond to rates from 10−4 to 104.   
Load  curve  ID  defining  failure  void  volume  fraction  𝑓𝐹  versus 
element length. 
Number of integration points which must fail before the element
is deleted.  This option is available for shells and solids. 
LT.0.0: |NUMINT|  is  percentage  of  integration  points/layers
which must fail before shell element fails.  For fully in-
tegrated  shells,  a  methodology  is  used  where  a  layer
fails  if  one  integration  point  fails  and  then  the  given
percentage  of  layers  must  fail  before  the  element  fails.
Only available for shells. 
LCF0 
Load  curve  ID  defining  initial  void  volume  fraction  𝑓0  versus 
element length.
LCFC 
LCFN 
*MAT_GURSON 
DESCRIPTION
Load  curve  ID  defining  critical  void  volume  fraction  𝑓𝑐  versus 
element length.   
Load  curve  ID  defining  void  volume  fraction  of  nucleating
particles 𝑓𝑁 versus element length.   
VGTYP 
Type of void growth behavior. 
EQ.0.0: Void growth in case of tension and void contraction in
case of compression, but never below 𝑓0 (default). 
EQ.1.0: Void growth only in case of tension. 
EQ.2.0: Void growth in case of tension and void contraction in 
case of compression, even below 𝑓0. 
DEXP 
Exponent value for damage history variable 16. 
Remarks: 
The Gurson flow function is defined as: 
Φ =
𝜎𝑀
2 + 2𝑞1𝑓 ∗cosh (
𝜎𝑌
3𝑞2𝜎𝐻
2𝜎𝑌
) − 1 − (𝑞1𝑓 ∗)2 = 0 
where  𝜎𝑀  is  the  equivalent  von  Mises  stress,  𝜎𝑌  is  the  yield  stress,  𝜎𝐻  is  the  mean 
hydrostatic stress.  The effective void volume fraction is defined as 
𝑓 ∗(𝑓 ) =
⎧𝑓
{
⎨
{
⎩
𝑓𝑐 +
1/𝑞1 − 𝑓𝑐
𝑓𝐹 − 𝑓𝑐
𝑓 ≤ 𝑓𝑐
(𝑓 − 𝑓𝑐)
𝑓 > 𝑓c
The growth of void volume fraction is defined as 
𝐺 + 𝑓 ̇
𝑁 
where the growth of existing voids is defined as 
𝑓 ̇ = 𝑓 ̇
𝑝  
𝑓 ̇
𝐺 = (1 − 𝑓 )𝜀̇𝑘𝑘
and nucleation of new voids is defined as 
𝑓 ̇
𝑁 = 𝐴𝜀̇𝑝 
with function A 
𝐴 =
𝑓𝑁
𝑆𝑁√2𝜋
exp [−
(
𝜀𝑝 − 𝜀𝑁
𝑆𝑁
)
] 
Voids are nucleated only in tension.
History variables: 
 Shell  /  Solid  Description   
1  /  1 
4  /  2 
5  /  3 
6  /  4 
7  /  5 
Void volume fraction  
Triaxiality variable σH/σM 
Effective strain rate 
Growth of voids 
Nucleation of voids 
11  /  11 
Dimensionless material damage value =
{⎧ (f−f0)
(fc−f0)
{⎨
1 +
⎩
(f−fc)
(fF−fc)
𝑓 ≤ 𝑓c
𝑓 > 𝑓c
13  /  13 
Deviatoric part of microscopic plastic strain 
14  /  14 
Volumetric part of macroscopic plastic strain 
16  /  16 
Dimensionless material damage value =   (
𝑓 −𝑓0
𝑓𝐹−𝑓0
1/DEXP
)
*MAT_GURSON_JC 
This is an enhancement of Material Type 120.  This is the Gurson model with additional 
Johnson-Cook  failure  criterion  (parameters  Card  5).    This  model  is  available  for  shell 
and solid elements. Strain rate dependency can be defined via a table.  An extension for 
void growth under shear-dominated states and for Johnson-Cook damage evolution is 
optional. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
SIGY 
F 
6 
N 
F 
7 
Q1 
F 
8 
Q2 
F 
Default 
none 
none 
none 
none 
none 
0.0 
none 
none 
  Card 2 
Variable 
Type 
Default 
1 
FC 
F 
0 
  Card 3 
1 
2 
F0 
F 
0 
2 
3 
EN 
F 
0 
3 
4 
SN 
F 
0 
4 
5 
FN 
F 
0 
5 
6 
7 
8 
ETAN 
ATYP 
FF0 
F 
0 
6 
F 
0 
7 
F 
0 
8 
Variable 
EPS1 
EPS2 
EPS3 
EPS4 
EPS5 
EPS6 
EPS7 
EPS8 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SIG1 
SIG2 
SIG3 
SIG4 
SIG5 
SIG6 
SIG7 
SIG8 
Type 
Default 
F 
0 
  Card 5 
1 
Variable 
LCDAM 
Type 
Default 
F 
0 
  Card 6 
1 
F 
0 
2 
L1 
F 
0 
2 
F 
0 
3 
L2 
F 
0 
3 
F 
0 
4 
D1 
F 
0 
4 
F 
0 
5 
D2 
F 
0 
5 
F 
0 
6 
D3 
F 
0 
6 
F 
0 
7 
D4 
F 
0 
7 
F 
0 
8 
LCJC 
F 
0 
8 
Variable 
LCSS 
LCFF 
NUMINT 
LCF0 
LCFC 
LCFN 
VGTYP 
DEXP 
Type 
Default 
F 
0 
F 
0 
F 
1 
F 
0 
F 
0 
F 
0 
F 
0 
F 
3.0 
Optional Card (starting with version 971 release R4)  
4 
5 
6 
7 
8 
  Card 7 
1 
2 
Variable 
KW 
BETA 
Type 
Default 
F 
0 
F 
0 
3 
M 
F 
1.0
VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
SIGY 
N 
Q1 
Q2 
FC 
F0 
EN 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
Yield stress. 
Exponent for Power law.  This value is only used if ATYP = 1 and 
LCSS = 0. 
Gurson flow function parameter 𝑞1. 
Gurson flow function parameter 𝑞2. 
Critical void volume fraction 𝑓𝑐 where voids begin to aggregate. 
Initial void volume fraction 𝑓0. This value is only used if LCF0 = 0.
Mean nucleation strain 𝜀𝑁.  
GT.0.0:  Constant value, 
LT.0.0:  Load  curve  ID = (-EN)  which  defines  mean  nucleation 
strain 𝜀𝑁  as a function of element length. 
SN 
Standard deviation 𝑠𝑁 of the normal distribution of 𝜀𝑁.  
GT.0.0:  Constant value, 
LT.0.0:  Load  curve 
ID = (-SN)  which  defines  standard 
deviation 𝑠𝑁 of the normal distribution of 𝜀𝑁 as a func-
tion of element length. 
FN 
ETAN 
Void volume fraction of nucleating particles𝑓𝑁. This value is only 
used if LCFN = 0. 
Hardening  modulus.    This  value  is  only  used  if  ATYP = 2  and 
LCSS = 0.
VARIABLE   
DESCRIPTION
ATYP 
Type of hardening. 
EQ.0.0: Ideal plastic, 
EQ.1.0: Power law, 
𝜎𝑌 = SIGY. 
𝜎𝑌 = SIGY × (
𝜀𝑝 + SIGY/E
SIGY/E
1/N
)
EQ.2.0: Linear hardening, 
𝜎𝑌 = SIGY +
E × ETAN
E − ETAN
𝜀𝑝. 
EQ.3.0: 8 points curve. 
FF0 
Failure  void  volume  fraction  𝑓𝐹.  This  value  is  only  used  if 
LCFF = 0. 
EPS1 - EPS8 
Effective  plastic  strain  values.    The  first  point  must  be  zero
corresponding to the initial yield stress.  At least 2 points should
be defined.  These values are used if ATYP = 3 and LCSS = 0. 
ES1 - ES8 
LCDAM 
L1 
L2 
Corresponding yield stress values to EPS1 – EPS8.  These values 
are used if ATYP = 3 and LCSS = 0. 
Load  curve  defining  scaling  factor  Λ  versus  element  length. 
Scales  the  Johnson-Cook  failure  strain  . 
  If 
LCDAM = 0, no scaling is performed. 
Lower triaxiality factor defining failure evolution (Johnson-Cook).
Upper triaxiality factor defining failure evolution (Johnson-Cook).
D1 - D4 
Johnson-Cook damage parameters. 
LCJC 
Load  curve  defining  scaling  factor  for  Johnson-Cook  failure 
versus  triaxiality  .    If  LCJC > 0,  parameters  D1,  D2 
and D3 are ignored.
VARIABLE   
LCSS 
LCFF 
NUMINT 
LCF0 
LCFC 
LCFN 
DESCRIPTION
Load  curve  ID  or  Table  ID.    ATYP  is  ignored  with  this  option.
Load  curve  ID  defining  effective  stress  versus  effective  plastic 
strain.  Table ID defines for each strain rate value a load curve ID
giving  the  effective  stress  versus  effective  plastic  strain  for  that
rate .   The stress-strain curve for the lowest value 
of  strain  rate  is  used  if  the  strain  rate  falls  below  the  minimum 
value.    Likewise,  the  stress-strain  curve  for  the  highest  value  of 
strain rate is used if the strain rate exceeds the maximum value. 
NOTE: The strain rate values defined in the table may be given as
the  natural  logarithm  of  the  strain  rate.    If  the  first  stress-strain 
curve in the table corresponds to a negative strain rate, LS-DYNA 
assumes that the natural logarithm of the strain rate value is used.
Since  the  tables  are  internally  discretized  to  equally  space  the
points,  natural  logarithms  are  necessary,  for  example,  if  the
curves correspond to rates from 10−4 to  104. 
Load  curve  ID  defining  failure  void  volume  fraction  𝑓𝐹  versus 
element length. 
Number  of  through  thickness  integration  points  which  must  fail 
before  the  element  is  deleted.    This  option  is  available  for  shells
and solids. 
LT.0.0: |NUMINT|  is  percentage  of  integration  points/layers
which must fail before shell element fails.  For fully in-
tegrated  shells,  a  methodology  is  used  where  a  layer
fails  if  one  integration  point  fails  and  then  the  given
percentage  of  layers  must  fail  before  the  element  fails. 
Only available for shells. 
Load  curve  ID  defining  initial  void  volume  fraction  𝑓0  versus 
element length. 
Load  curve  ID  defining  critical  void  volume  fraction  𝑓𝑐  versus 
element length. 
Load  curve  ID  defining  void  volume  fraction  of  nucleating 
particles 𝑓𝑁 versus element length.
VARIABLE   
DESCRIPTION
VGTYP 
Type of void growth behavior. 
EQ.0.0: Void growth in case of tension and void contraction in
case of compression, but never below 𝑓0 (default). 
EQ.1.0: Void growth only in case of tension. 
EQ.2.0: Void growth in case of tension and void contraction in
case of compression, even below 𝑓0. 
DEXP 
Exponent value for damage history variable 16. 
KW 
Parameter  kω  for  void  growth  in  shear-dominated  states.    See 
remarks. 
BETA 
Parameter β in Lode cosine function.  See remarks. 
M 
Parameter for generalization of Johnson-Cook damage evolution. 
See remarks. 
Remarks: 
The Gurson flow function is defined as: 
Φ =
𝜎𝑀
2 + 2𝑞1𝑓 ∗cosh (
𝜎𝑌
3𝑞2𝜎𝐻
2𝜎𝑌
) − 1 − (𝑞1𝑓 ∗)2 = 0 
where  𝜎𝑀  is  the  equivalent  von  Mises  stress,  𝜎𝑌  is  the  yield  stress,  𝜎𝐻  is  the  mean 
hydrostatic stress.  The effective void volume fraction is defined as 
𝑓 ∗(𝑓 ) =
⎧𝑓
{
⎨
{
⎩
𝑓𝑐 +
1/𝑞1 − 𝑓𝑐
𝑓𝐹 − 𝑓𝑐
𝑓 ≤ 𝑓𝑐
(𝑓 − 𝑓𝑐)
𝑓 > 𝑓c
The growth of void volume fraction is defined as 
𝐺 + 𝑓 ̇
𝑁 
where the growth of existing voids is defined as 
𝑓 ̇ = 𝑓 ̇
𝑓 ̇
𝐺 = (1 − 𝑓 )𝜀̇𝑘𝑘
𝑝 + 𝑘𝜔𝜔(σ)𝑓 (1 − 𝑓 )𝜀̇𝑀
𝑝𝑙 𝜎𝑌
𝜎𝑀
The  second  term  is  an  optional  extension  for  shear  failure  proposed  by  Nahshon  and 
Hutchinson [2008] with new parameter 𝑘𝜔 (=0 by default), effective plastic strain rate in 
the matrix 𝜀̇𝑀
𝑝𝑙 , and Lode cosin function 𝜔(σ): 
𝜔(σ) = 1 − 𝜉 2 − 𝛽 ⋅ 𝜉 (1 − 𝜉 ),        𝜉 = cos(3𝜃) =
27
𝐽3
3  
𝜎𝑀
with parameter 𝛽, Lode angle 𝜃 and third deviatoric stress invariant 𝐽3. 
Nucleation of new voids is defined as 
𝑝𝑙  
𝑓 ̇
𝑁 = 𝐴𝜀̇𝑀
with function A 
𝐴 =
𝑓𝑁
𝑆𝑁√2𝜋
exp
⎜⎜⎛𝜀𝑀
2 ⎝
𝑝𝑙 − 𝜀𝑁
⎟⎟⎞
𝑆𝑁 ⎠
⎡
−
⎢⎢
⎣
⎤
⎥⎥
⎦
Voids are nucleated only in tension. 
The  Johnson-Cook  failure  criterion  is  added  in  this  material  model.    Based  on  the 
triaxiality ratio 𝜎𝐻/𝜎𝑀 failure is calculated as: 
𝜎𝐻/𝜎𝑀 > 𝐿1  : Gurson model 
𝐿1 ≥ 𝜎𝐻/𝜎𝑀 ≥ 𝐿2  : Gurson model and Johnson-Cook failure criteria 
𝐿2 < 𝜎𝐻/𝜎𝑀 
: Gurson model 
Johnson-Cook failure strain is defined as 
𝜀𝑓 = [𝐷1 + 𝐷2exp (𝐷3
𝜎𝐻
𝜎𝑀
)] (1 + 𝐷4ln 𝜀̇)Λ 
where 𝐷1, 𝐷2, 𝐷3 and 𝐷4 are the Johnson-Cook failure parameters and Λ is a function 
for including mesh-size dependency.  An alternative expression can be used, where the 
first  term  of  the  above  equation  (including  D1,  D2  and  D3)  is  replaced  by  a  general 
function LCJC which depends on triaxiality 
𝜎𝐻
𝜎𝑀
) (1 + 𝐷4ln𝜀̇)Λ 
𝜀𝑓 = LCJC × (
The  Johnson-Cook  damage  parameter  𝐷𝑓   is  calculated  with  the  following  evolution 
equation: 
𝐷̇ 𝑓 =
𝜀̇𝑝𝑙
𝜀𝑓
⇒ 𝐷𝑓 = ∑
Δ𝜀𝑝𝑙
𝜀𝑓
. 
where  𝛥𝜀𝑝𝑙  is  the  increment  in  effective  plastic  strain.    The  material  fails  when  𝐷𝑓  
reaches  1.0.    A  more  general  (non-linear)  damage  evolution  is  possible  if  𝑀 > 1  is 
chosen: 
𝐷̇ 𝑓 =
(1− 1
𝐷𝑓
)
𝜀̇𝑝𝑙,
𝜀𝑓
𝑀 ≥ 1.0
Shell  /  Solid  Description 
*MAT_120_JC 
1  /  1 
4  /  2 
5  /  3 
6  /  4 
7  /  5 
8  /  6 
9  /  7 
0  /  8 
Void volume fraction  
Triaxiality variable σH/σM 
Effective strain rate 
Growth of voids 
Nucleation of voids 
Johnson-Cook failure strain εf 
Johnson-Cook damage parameter Df 
Domain variable: 
EQ.0   elastic stress update 
EQ.1   region (a) Gurson 
EQ.2   region (b) Gurson + Johnson-Cook 
EQ.3   region (c) Gurson 
11  /  11 
Dimensionless material damage value =
{⎧ (f−f0)
(fc−f0)
{⎨
1 +
⎩
(f−fc)
(fF−fc)
𝑓 ≤ 𝑓c
𝑓 > 𝑓c
13  /  13 
Deviatoric part of microscopic plastic strain  
14  /  14  
Volumetric part of macroscopic plastic strain 
16  /  16 
Dimensionless material damage value = (
1/DEXP
f−f0
fF−f0
)
*MAT_GURSON_RCDC 
This  is  an  enhancement  of  material  Type  120.    This  is  the  Gurson  model  with  the 
Wilkins Rc-Dc [Wilkins, et al., 1977] fracture model added.  This model is available for 
shell  and  solid  elements.    A  detailed  description  of  this  model  can  be  found  in  the 
following  references:  Gurson  [1975,  1977];  Chu  and  Needleman  [1980];  and  Tvergaard 
and Needleman [1984]. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
SIGY 
F 
6 
N 
F 
7 
Q1 
F 
8 
Q2 
F 
Default 
none 
none 
none 
none 
none 
0.0 
none 
none 
  Card 2 
Variable 
Type 
Default 
1 
FC 
F 
0 
  Card 3 
1 
2 
F0 
F 
0 
2 
3 
EN 
F 
0 
3 
4 
SN 
F 
0 
4 
5 
FN 
F 
0 
5 
6 
7 
8 
ETAN 
ATYP 
FF0 
F 
0 
6 
F 
0 
7 
F 
0 
8 
Variable 
EPS1 
EPS2 
EPS3 
EPS4 
EPS5 
EPS6 
EPS7 
EPS8 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ES1 
ES2 
ES3 
ES4 
ES5 
ES6 
ES7 
ES8 
Type 
Default 
  Card 5 
Variable 
Type 
Default 
F 
0 
1 
L1 
F 
0 
  Card 6 
1 
F 
0 
2 
L2 
F 
0 
2 
F 
0 
3 
L3 
F 
0 
3 
Variable 
LCSS 
LCLF 
NUMINT 
Type 
Default 
F 
0 
  Card 7 
1 
F 
0 
2 
F 
1 
3 
F 
0 
4 
L4 
F 
0 
4 
4 
Variable 
ALPHA 
BETA 
GAMMA 
D0 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
5 
F 
0 
6 
F 
0 
7 
F 
0 
8 
FF1 
FF2 
FF3 
FF4 
F 
0 
5 
5 
B 
F 
0 
F 
0 
6 
F 
0 
7 
6 
7 
LAMBDA 
DS 
F 
0 
F 
0 
F 
0 
8 
8 
L 
F
VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
SIGY 
N 
Q1 
Q1 
FC 
F0 
EN 
SN 
FN 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
Yield stress. 
Exponent for Power law.  This value is only used if ATYP = 1 and 
LCSS = 0. 
Parameter 𝑞1. 
Parameter 𝑞2. 
Critical void volume fraction 𝑓𝑐 
Initial void volume fraction 𝑓0. 
Mean nucleation strain𝜀𝑁. 
Standard deviation 𝑆𝑁 of the normal distribution of 𝜀𝑁. 
Void volume fraction of nucleating particles. 
ETAN 
Hardening  modulus.    This  value  is  only  used  if  ATYP = 2  and 
LCSS = 0. 
ATYP 
Type of hardening. 
EQ.0.0: Ideal plastic, 
EQ.1.0: Power law, 
𝜎𝑌 = SIGY. 
𝜎𝑌 = SIGY × (
𝜀𝑝 + SIGY/E
SIGY/E
1/N
)
EQ.2.0: Linear hardening, 
𝜎𝑌 = SIGY +
E × ETAN
E − ETAN
𝜀𝑝. 
EQ.3.0:  8 points curve. 
FF0 
Failure  void  volume  fraction.    This  value  is  used  if  no  curve  is
given by the points (L1, FF1) – (L4, FF4) and LCLF = 0.
VARIABLE   
EPS1 - EPS8 
DESCRIPTION
Effective  plastic  strain  values.    The  first  point  must  be  zero
corresponding to the initial yield stress.  This option is only used
if  ATYP  equal  to  3.    At  least  2  points  should  be  defined.    These
values are used if ATYP = 3 and LCSS = 0. 
ES1 - ES8 
Corresponding  yield  stress  values  to  EPS1  -  EPS8.    These  values 
are used if ATYP = 3 and LCSS = 0. 
L1 - L4 
Element length values.  These values are only used if LCLF = 0. 
FF1 - FF4 
Corresponding  failure  void  volume  fraction.    These  values  are
only used if LCLF = 0. 
LCSS 
LCLF 
Load  curve  ID  defining  effective  stress  versus  effective  plastic
strain.  ATYP is ignored with this option. 
Load  curve  ID  defining  failure  void  volume  fraction  versus
element  length.    The  values  L1  -  L4  and  FF1  -  FF4  are  ignored 
with this option. 
NUMINT 
Number  of  through  thickness  integration  points  which  must  fail
before the element is deleted. 
ALPHA 
Parameter 𝛼. for the Rc-Dc model 
BETA 
Parameter𝛽. for the Rc-Dc model 
GAMMA 
Parameter 𝛾. for the Rc-Dc model 
D0 
B 
Parameter 𝐷0. for the Rc-Dc model 
Parameter 𝑏. for the Rc-Dc model 
LAMBDA 
Parameter 𝜆. for the Rc-Dc model 
Parameter 𝐷𝑠. for the Rc-Dc model 
Characteristic element length for this material 
DS 
L 
Remarks: 
The Gurson flow function is defined as: 
Φ =
𝜎𝑀
2 + 2𝑞1𝑓 ∗cosh (
𝜎𝑌
3𝑞2𝜎𝐻
2𝜎𝑌
) − 1 − (𝑞1𝑓 ∗)2 = 0
where  𝜎𝑀  is  the  equivalent  von  Mises  stress,  𝜎𝑌  is  the  Yield  stress,  𝜎𝐻  is  the  mean 
hydrostatic stress.  The effective void volume fraction is defined as 
𝑓 ∗(𝑓 ) =
⎧𝑓
{
⎨
{
⎩
𝑓𝑐 +
1/𝑞1 − 𝑓𝑐
𝑓𝐹 − 𝑓𝑐
𝑓 ≤ 𝑓𝑐
(𝑓 − 𝑓𝑐)
𝑓 > 𝑓c
The growth of the void volume fraction is defined as 
where the growth of existing voids is given as: 
𝑓 ̇ = 𝑓 ̇
𝐺 + 𝑓 ̇
𝑁 
and nucleation of new voids as: 
in which 𝐴 is defined as 
𝑝 , 
𝑓 ̇
𝐺 = (1 − 𝑓 )𝜀̇𝑘𝑘
𝑓 ̇
𝑁 = 𝐴𝜀̇𝑝 
𝐴 =
𝑓𝑁
𝑆𝑁√2𝜋
exp (−
(
𝜀𝑝 − 𝜀𝑁
𝑆𝑁
)
) 
The Rc-Dc model is defined as the following: 
The damage 𝐷 is given by 
where 𝜀𝑝 is the equivalent plastic strain,  
𝐷 = ∫ 𝜔1𝜔2𝑑𝜀𝑝 
𝜔1 = (
1 − 𝛾𝜎𝑚
)
is a triaxial stress weighting term and 
𝜔2 = (2 − 𝐴𝐷)𝛽 
is a asymmetric strain weighting term. 
In the above 𝜎𝑚 is the mean stress and  
𝐴𝐷 = max (
𝑆2
𝑆3
,
𝑆2
𝑆1
) 
Fracture is initiated when the accumulation of damage is 
𝐷𝑐
> 1 
where 𝐷𝑐 is the a critical damage given by 
𝐷𝑐 = 𝐷0(1 + 𝑏|∇𝐷|𝜆)
*MAT_120_RCDC 
𝐹 =
𝐷 − 𝐷𝑐
𝐷𝑠
defines the degradations of the material by the Rc-Dc model. 
The  characteristic  element  length  is  used  in  the  calculation  of  ∇𝐷.  Calculation  of  this 
factor is only done for element with smaller element length than this value.
*MAT_GENERAL_NONLINEAR_1DOF_DISCRETE_BEAM 
This is Material Type 121.  This is a very general spring and damper model.  This beam 
is  based  on  the  MAT_SPRING_GENERAL_NONLINEAR  option  and  is  a  one-
dimensional  version  of  the  6DOF_DISCRETE_BEAM  above.    The  forces  generated  by 
this  model  act  along  a  line  between  the  two  connected  nodal  points.    Additional 
unloading options have been included. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
K 
F 
3 
4 
5 
6 
7 
8 
IUNLD 
OFFSET 
DAMPF 
I 
4 
F 
5 
F 
6 
7 
8 
Variable 
LCIDT 
LCIDTU 
LCIDTD 
LCIDTE 
Type 
I 
  Card 3 
1 
I 
2 
Variable 
UTFAIL 
UCFAIL 
Type 
F 
F 
I 
3 
IU 
F 
I 
4 
5 
6 
7 
8 
  VARIABLE   
DESCRIPTION
MID 
RO 
K 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density, see also volume in *SECTION_BEAM definition. 
Translational stiffness for unloading option 2.0.
VARIABLE   
DESCRIPTION
IUNLD 
Unloading option (Also see Figure M119-1): 
EQ.0.0: Loading and unloading follow loading curve 
EQ.1.0: Loading  follows  loading  curve,  unloading  follows
unloading curve.  The unloading curve ID if undefined
is taken as the loading curve. 
EQ.2.0: Loading  follows  loading  curve,  unloading  follows
unloading  stiffness,  K,  to  the  unloading  curve.    The
loading and unloading curves may only intersect at the 
origin of the axes. 
EQ.3.0: Quadratic unloading from peak displacement value to
a permanent offset. 
Offset  to  determine  permanent  set  upon  unloading  if  the
IUNLD = 3.0.  The permanent sets in compression and tension are 
equal  to  the  product  of  this  offset  value  and  the  maximum
compressive and tensile displacements, respectively. 
Damping factor for stability.  Values in the neighborhood of unity
are  recommended.    This  damping  factor  is  properly  scaled  to 
eliminate time step size dependency.  Also, it is active if and only
if the local stiffness is defined. 
Load curve ID defining translational force resultant along the axis
versus  relative  translational  displacement.    If  zero,  no  stiffness
related  forces  are  generated  for  this  degree  of  freedom.    The
loading  curves  must  be  defined  from  the  most  negative
displacement  to  the  most  positive  displacement.    The  force  does
not  need  to  increase  monotonically  for  the  loading  curve.    The
curves  are  extrapolated  when  the  displacement  range  falls 
outside the curve definition. 
Load curve ID defining translational force resultant along the axis
versus relative translational displacement during unloading.  The
force  values  defined  by  this  curve  must  increase  monotonically 
from  the  most  negative  displacement  to  the  most  positive
displacement.    For  IUNLD = 1.0,  the  slope  of  this  curve  must 
equal or exceed the loading curve for stability reasons.  This is not
the  case  for  IUNLD = 2.0.    For  loading  and  unloading  to  follow 
the same path simply set LCIDTU = LCIDT. 
OFFSET 
DAMPF 
LCIDT 
LCIDTU 
LCIDTD 
Load  curve  ID  defining  translational  damping  force  resultant
along the axis versus relative translational velocity.
LCIDTE 
UTFAIL 
UCFAIL 
*MAT_GENERAL_NONLINEAR_1DOF_DISCRETE_BEAM 
DESCRIPTION
Load  curve  ID  defining  translational  damping  force  scale  factor
versus relative displacement along the axis. 
Optional, translational displacement at failure in tension.  If zero,
failure in tension is not considered. 
Optional, translational displacement at failure in compression.  If
zero, failure in compression is not considered. 
IU 
Initial translational displacement along axis.
*MAT_122 
This is Material Type 122.  This is Hill’s 1948 planar anisotropic material model with 3 R 
values. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
E 
F 
3 
4 
PR 
F 
4 
Variable 
R00 
R45 
R90 
LCID 
F 
2 
F 
3 
Type 
F 
  Card 3 
1 
Variable 
AOPT 
Type 
F 
  Card 4 
1 
2 
3 
Variable 
Type 
  Card 5 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
F 
4 
4 
A1 
F 
4 
D1 
F 
5 
HR 
F 
5 
E0 
F 
5 
5 
A2 
F 
5 
D2 
F 
6 
P1 
F 
6 
7 
P2 
F 
7 
8 
8 
6 
7 
8 
6 
A3 
F 
6 
D3 
F 
7 
8 
7 
8 
BETA
MID 
RO 
E 
PR 
HR 
*MAT_HILL_3R 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus, E 
Poisson’s ratio, ν 
Hardening rule: 
EQ.1.0:  linear (default), 
EQ.2.0:  exponential. 
EQ.3.0:  load curve 
P1 
Material parameter: 
HR.EQ.1.0: Tangent modulus, 
HR.EQ.2.0: k, strength coefficient for exponential hardening 
P2 
Material parameter: 
HR.EQ.1.0: Yield stress 
HR.EQ.2.0: n, exponent 
R00 
R45 
R90 
R00, Lankford parameter determined from experiments 
R45, Lankford parameter determined from experiments 
R90, Lankford parameter determined from experiments 
LCID 
load curve ID for the load curve hardening rule 
E0 
𝜀0  for  determining  initial  yield  stress  for  exponential  hardening.
(Default = 0.0)
AOPT 
*MAT_122 
DESCRIPTION
Material axes option : 
EQ.0.0:  locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES,  and  then  rotated  about  the  shell  ele-
ment normal by an angle BETA. 
EQ.2.0:  globally  orthotropic  with  material  axes  determined  by
the  vector  a  defined  below,  as  with  *DEFINE_COOR-
DINATE_VECTOR. 
EQ.3.0:  locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the 
element normal. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
XP YP ZP 
Coordinates of point p for AOPT = 1. 
A1 A2 A3 
Components of vector a for AOPT = 2. 
V1 V2 V3 
Components of vector v for AOPT = 3. 
D1 D2 D3 
Components of vector d for AOPT = 2. 
BETA 
Μaterial angle in degrees for AOPT = 0 and 3, may be overridden 
on the element card, see *ELEMENT_SHELL_BETA. 
Remarks: 
The calculated effective stress is stored in history variable #4.
*MAT_HILL_3R_3D 
This is Material Type 122_3D.  It combines orthotropic elastic behavior with Hill’s 1948 
anisotropic  plasticity  theory.    Anisotropic  plastic  properties  are  given  by  6  material 
parameters,  𝐹,  𝐺,  𝐻,  𝐿,  𝑀,  𝑁  which  are  determined  by  experiments.    This  model  is 
implemented for solid elements. 
This keyword can be written either as *MAT_HILL_3R_3D, or *MAT_122_3D. 
  Card 1 
1 
Variable 
MID 
Type 
I 
  Card 2 
1 
2 
RO 
F 
2 
3 
EX 
F 
3 
Variable 
GXY 
GYZ 
GXZ 
Type 
F 
F 
F 
2 
HR 
I 
2 
3 
P1 
I/F 
3 
  Card 3 
Variable 
Type 
1 
N 
F 
  Card 4 
1 
Variable 
AOPT 
Type 
I 
4 
EY 
F 
4 
F 
F 
4 
P2 
F 
4 
5 
EZ 
F 
5 
G 
F 
5 
6 
7 
8 
PRXY 
PRYZ 
PRXZ 
F 
6 
H 
F 
6 
F 
7 
L 
F 
7 
F 
8 
M 
F 
8 
5 
6 
7
Card 5 
Variable 
1 
XP 
Type 
F 
  Card 6 
Variable 
1 
V1 
Type 
F 
2 
YP 
F 
2 
V2 
F 
3 
ZP 
F 
3 
V3 
F 
4 
A1 
F 
4 
D1 
F 
5 
A2 
F 
5 
D2 
F 
6 
A3 
F 
6 
D3 
F 
7 
8 
7 
8 
BETA 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
EX, EY, EZ 
Material identification ID, must be a unique number. 
Mass density. 
Young’s  modulus  in  𝑥,  𝑦,  and  𝑧  directions,  respectively.
Negative  values  indicate  (positive)  curve  numbers,  where
each curve is a function of temperature.  
PRXY, PRYZ, PRXZ 
Poisson’s  ratio,  𝜈,  in  𝑥𝑦,  𝑦𝑧  and  𝑥𝑧  directions,  respectively. 
Negative  values  indicate  (positive)  curve  numbers,  where
each curve is a function of temperature. 
GXY, GYZ, GXZ 
F, G, H, L, M, N 
Shear  modulus  in  𝑥𝑦,  𝑦𝑧  and  𝑥𝑧  directions,  respectively. 
Negative  values  indicate  (positive)  curve  numbers,  where 
each curve is a function of temperature. 
Material  constants  in  Hill’s  1948  yield  criterion  . 
  Negative  values  indicate  (positive)  curve
numbers, where each curve is a function of temperature. 
HR 
Hardening rule: 
EQ.1:  Stress-strain  relationship  is  defined  by  load  curve 
or 2D-table ID with parameter P1.  P2 is ignored. 
EQ.2:  Stress-strain  relationship  is  defined  by  strength 
coefficient  K  (P1)  and  strain  hardening  coefficient
n  (P2),  as  in  Swift’s  exponential  hardening  equa-
tion: 𝜎yield = 𝑘(𝜀 + 0.01)𝑛.
VARIABLE   
DESCRIPTION
P1 
Material parameter: 
HR.EQ.1:  Load  curve  or  2D-table  ID  defining  stress-
strain  curve.    If  2D-table  ID,  the  table  gives 
stress-strain curves for different temperatures.
HR.EQ.2:  𝑘, strength coefficient in 𝜎yield = 𝑘(𝜀 + 0.01)𝑛. 
P2 
Material parameter: 
HR.EQ.1:  not used. 
HR.EQ.2.0:  𝑛, the exponent in 𝜎𝑦𝑖𝑒𝑙𝑑 = 𝑘(𝜀 + 0.01)𝑛. 
AOPT 
Material axes option : 
EQ.0.0:  locally 
orthotropic  with  material 
axes 
determined by element nodes 1, 2, and 4, as with
*DEFINE_COORDINATE_NODES. 
EQ.1.0:  locally 
orthotropic  with  material 
axes
determined by a point 𝐩 in space and the global 
location  of  the  element  center;  this  is  the  a-
direction.  This option is for solid elements only.
EQ.2.0:  globally 
orthotropic  with  material 
axes
determined by the vectors 𝐚 and 𝐝, as with *DE-
FINE_COORDINATE_VECTOR. 
EQ.3.0:  locally  orthotropic  material  axes  determined  by 
rotating  the  material  axes  about  the  element
normal  by  an  angle,  BETA,  from  a  line  in  the
plane of the element defined by the cross prod-
uct of the vector 𝐯 with the element normal. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate
system ID number (CID on *DEFINE_COORDI-
NATE_NODES,  *DEFINE_COORDINATE_SYS-
TEM or *DEFINE_COORDINATE_VECTOR). 
XP, YP, ZP 
Coordinates of point 𝐩 for AOPT = 1. 
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3. 
D1, D2, D3 
Components of vector 𝐝 for AOPT = 2.
BETA 
*MAT_122_3D 
DESCRIPTION
Material angle in degrees for AOPT = 3, may be overridden 
on the element card, see *ELEMENT_SHELL_BETA or *EL-
EMENT_SOLID_ORTHO. 
Hill’s 1948 yield criterion: 
Hill’s  yield  criterion  is  based  on  the  assumptions  that  the  material  is  orthotropic,  that 
hydrostatic  stress  does  not  affect  yielding,  and  that  there  is  no  Bauschinger  effect.  
According  to  Hill,  when  the  principal  axes of anisotropy  are the axes  of reference,  the 
yield surface has the form 
where the effective stress 𝜎̅̅̅̅̅ (stored as history variable #2) is given by 
𝑓 = 𝜎̅̅̅̅̅(𝝈) − 𝜎yield(𝜀𝑝) = 0, 
(𝐹 + 𝐺)𝜎̅̅̅̅̅ 2 = 𝐹(𝜎𝑦 − 𝜎𝑧)
+ 𝐺(𝜎𝑧 − 𝜎𝑥)2 + 𝐻(𝜎𝑥 − 𝜎𝑦)
+ 2𝐿𝜏𝑦𝑧
2 + 2𝑀𝜏𝑧𝑥
2 , 
2 + 2𝑁𝜏𝑥𝑦
and where 𝐹, 𝐺, 𝐻, 𝐿, 𝑀, 𝑁 are material parameters of the current state of anisotropy, 
assuming three mutually orthogonal planes of symmetry at every point.  The material 𝑧-
direction is here the reference direction. 
Let 𝑋, 𝑌, 𝑍 be the tensile yield stresses in the principal directions of anisotropy, then 
𝜎y0
𝑋2 =
𝐺 + 𝐻
𝐹 + 𝐺
,
𝜎y0
𝑌2 =
𝐻 + 𝐹
𝐹 + 𝐺
,
𝜎y0
𝑍2 = 1, 
where  𝜎y0 = 𝜎yield(0).  𝐹,  𝐺,  𝐻  are  not  uniquely  determined,  but  the  choice  F+G = 1 
gives 
𝐹 =
𝑍2
(
𝑌2 +
𝑍2 −
𝑋2) ,
𝐺 =
𝑍2
𝑋2 +
(
𝑍2 −
𝑌2) ,
𝐻 =
𝑍2
(
𝑋2 +
𝑌2 −
𝑍2).
Material 
F 
G 
H 
L 
M 
N 
AA5042 
0.3341 
0.5098 
0.3569 
1.5000 
1.5000 
1.8197 
Table  M122-1. 
NUMISHEET 2011. 
  AA5042  material  constants  (Hill’s  1948  yield)  -  BM1
If  𝑅𝑥𝑦  ,  𝑆𝑧𝑥  ,  𝑇𝑥𝑦  are  the  yield  stresses  in  shear  with  respect  to  the  principal  axes  of 
anisotropy, then 
𝐿 =
𝑍2
2 ,
2𝑅𝑥𝑦
𝑀 =
𝑍2
2 ,
2𝑆𝑧𝑥
𝑁 =
𝑍2
2 . 
2𝑇𝑥𝑦
If  𝐹 = 𝐺 = 𝐻,  and,  𝐿 = 𝑀 = 𝑁 = 3𝐹,  the  Hill  criterion  reduces  to  the  Von-Mises 
criterion. 
The  strain  hardening  in  this  model  can  either  defined  by  the  load  curve  or  by  Swift’s 
exponential hardening equation: 𝜎yield = 𝑘(𝜀 + 0.01)𝑛. 
Validation and application: 
1.  This  material  model  is  suitable  for  metal  forming  application  using  solid 
elements  to  account  for  anisotropic  plasticity.    NUMISHEET  conferences  have 
provided material constants of Hill’s 1948 yield for many commonly used ma-
terials.  In this example, experimental results from benchmark 1 (BM1, AA5042) 
of the NUMISHEET 2011 are used to validate an equal-biaxial tension and two 
uniaxial  tensile  results  in  two  different  directions  (rolling  and  90°)  on  a  single 
solid element. 
As  shown  in  Figure  M122-1(top  left),  under  the  constraints  imposed,  a  single 
element  of  solid  type  2  is  pulled  in  uniaxial  tension  in  the  𝑥-direction.    The 
resulting  hardening  curve  is  compared  with  experimental  data  provided  (top 
right).    Similarly,  the  element  is  pulled  in  uniaxial  tension  in  the  Y-direction 
under the constraints shown in Figure M122-1(middle left).  The resulting hard-
ening  curve  is  compared  with  experimental  data  (middle  right).    In  Figure 
M122-1(bottom  left),  the  element  is  pulled  in  both  𝑥-  and  𝑦-directions  equally
under  the  constraints  shown,  and  the  resulting  hardening  curve  is  compared 
with  experimental  data  (bottom  right).    All  computed  results  are  satisfactory.  
The material constants used for the simulation are provided in Table M122-1.  
In  addition,  an  element  of  type  1  is  subjected  to  a  shear  test  with  a  composite 
material,  courtesy  of  CYBERNET  SYSTEMS  CO.,  LTD.    Results  compare  well 
with the experiments, as shown in Figure M122-2. 
In real world application, the six material parameters required can be calibrated 
with  nonlinear  regression  analysis  (such  as  those  available  through  LS-OPT) 
through  a  series  of  tensile  tests  in  three  orthogonal  directions  and  three  shear 
tests in three orthogonal planes. 
2.  This material model can also be applied in multi-scale simulation of fiberglass 
and  laminated  materials,  according  to  CYBERNET  SYSTEMS  CO.,  LTD.    The 
elastic  coefficients  can  be  calibrated  analytically  by  a  homogenization  method 
with tensile tests in the three orthogonal directions and three pure shear tests in 
the three orthogonal planes. 
Revision information: 
The material model is available in explicit dynamics in both SMP and MPP starting in 
Revision 86100, and is available in implicit dynamics in both SMP and MPP starting in 
Revision  104178.    It  also  supports  temperature  dependent  Young’s/shear  modulus, 
Poisson ratios, and Hill parameters.
0=
*MAT_HILL_3R_3D 
Rolling direction (0 deg.) tensile pull
ux
Fy
0=
)
(
500.0
400.0
300.0
200.0
100.0
0.0
)
(
500.0
400.0
300.0
200.0
100.0
0.0
)
(
500.0
400.0
300.0
200.0
100.0
0.0
Fz
0=
Fz
0=
uy
ux
uy
Experiment
LS-DYNA
0.0 0.03
0.08
0.13
0.18
True strain
90 deg. tensile pull
Experiment
LS-DYNA
0.0 0.03
0.08
0.13
0.18
True strain
Equi-biaxial test
Experiment
LS-DYNA
0.0 0.03
0.08
0.13
0.18
True strain
Fy
0=
Figure M122-1.  Validation with experiments - BM1 NUMISHEET 2011
ux
35.0
30.0
25.0
20.0
10.0
)
(
0.0
0.0
XY shear test
Experiment
LS-DYNA
0.01
0.02
0.03
True strain
Figure  M122-2.    Shear  result  validated  with  test  results  (Courtesy  of
CYBERNET SYSTEMS CO., LTD.)
*MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY_{OPTION} 
This  is  Material  Type  123,  which  is  an  elasto-plastic  material  supporting  an  arbitrary 
stress  versus  strain  curve  as  well  as  arbitrary  strain  rate  dependency.    This  model  is 
available  for  shell  and  solid  elements.    Another  model,  MAT_PIECEWISE_LINEAR_
PLASTICITY,  is  similar  but  lacks  the  enhanced  failure  criteria.    Failure  is  based  on 
effective plastic strain, plastic thinning, the major principal in plane strain component, 
or a minimum time step size.  See the discussion under the model description for MAT_
PIECEWISE_LINEAR_PLASTICITY if more information is desired. 
Available options include: 
<BLANK> 
RATE 
RTCL 
STOCHASTIC (for shells only) 
The  “RATE”  option  is  used  to  account  for  rate  dependence  of  plastic  thinning  failure.  
The  “RTCL”  option  is  used  to  activate  RTCL  damage.    One  additional  card  is  needed 
with either option. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
6 
7 
8 
SIGY 
ETAN 
FAIL 
TDEL 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
0.0 
10.E+20 
  Card 2 
Variable 
Type 
Default 
1 
C 
F 
0 
2 
P 
F 
0 
3 
4 
5 
6 
7 
LCSS 
LCSR 
VP 
EPSTHIN 
EPSMAJ  NUMINT 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0
Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EPS1 
EPS2 
EPS3 
EPS4 
EPS5 
EPS6 
EPS7 
EPS8 
Type 
Default 
F 
0 
  Card 4 
1 
F 
0 
2 
F 
0 
3 
F 
0 
4 
F 
0 
5 
F 
0 
6 
F 
0 
7 
F 
0 
8 
Variable 
ES1 
ES2 
ES3 
ES4 
ES5 
ES6 
ES7 
ES8 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
Card 5 is required if and only if either the RATE or RTCL option is active.  
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCTSRF 
EPS0 
TRIAX 
Type 
Default 
I 
0 
F 
0 
F 
0 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
SIGY 
Yield stress.
*MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY 
DESCRIPTION
ETAN 
Tangent modulus, ignored if (LCSS.GT.0) is defined. 
FAIL 
Failure flag. 
LT.0.0:  User defined failure subroutine, matusr_24 in dyn21.F, 
is called to determine failure 
EQ.0.0: Failure is not considered.  This option is recommended
if failure is not of interest since many calculations will
be saved. 
GT.0.0:  Plastic strain to failure.  When the plastic strain reaches
this value, the element is deleted from the calculation. 
TDEL 
Minimum time step size for automatic element deletion. 
C 
P 
Strain rate parameter, C, see formula below. 
Strain rate parameter, P, see formula below. 
LCSS 
Load curve ID or Table ID. 
Load  Curve.    When  LCSS  is  a  Load  curve  ID,  it  is  taken  as
defining effective stress versus effective plastic strain.  If defined
EPS1 - EPS8 and ES1 - ES8 are ignored. 
Tabular  Data.    The  table  ID  defines  for  each  strain  rate  value  a
load  curve  ID  giving  the  stress  versus  effective  plastic  strain  for 
that rate, See Figure M24-1.  When the strain rate falls below the 
minimum value, the stress versus effective plastic strain curve for
the lowest value of strain rate is used.  Likewise, when the strain 
rate exceeds the maximum value the stress versus effective plastic
strain curve for the highest value of strain rate is used.  The strain
rate  parameters:  C  and  P,  the  curve  ID,  LCSR,  EPS1 -  EPS8,  and 
ES1 - ES8 are ignored if a Table ID is defined. 
Logarithmically Defined Tables.  If the first stress-strain curve in 
the table corresponds to a negative strain rate, LS-DYNA assumes 
that  the  natural  logarithm  of  the  strain  rate  value  is  used  for  all
stress-strain curves.   Since the tables are internally discretized to
equally  space  the  points,  natural  logarithms  are  necessary,  for
example,  if  the  curves  correspond  to  rates  from  10−4  to  104. 
Computing  natural  logarithms  can  substantially  increase  the
computational time on certain computer architectures. 
LCSR 
Load curve ID defining strain rate scaling effect on yield stress.
VARIABLE   
DESCRIPTION
VP 
Formulation for rate effects: 
EQ.0.0: Scale yield stress (default), 
EQ.1.0: Viscoplastic formulation (recommended). 
EPSTHIN 
Thinning  strain  at  failure.    This  number  should  be  given  as  a
positive number. 
EPSMAJ 
Major in plane strain at failure. 
NUMINT 
EPS1 - EPS8 
LT.0: EPSMAJ = |EPSMAJ| and filtering is activated.  The last
twelve values of the major strain is stored at each integra-
tion  point  and  the  average  value  is  used  to  determine
failure. 
Number of integration points which must fail before the element
is deleted.  (If zero, all points must fail.)  For fully integrated shell
formulations,  each  of  the  4 × NIP  integration  points  are  counted 
individually  in  determining  a  total  for  failed  integration  points.
NIP  is  the  number  of  through-thickness  integration  points.    As 
NUMINT approaches the total number of integration points (NIP
for under integrated shells, 4*NIP for fully integrated shells), the
chance of instability increases. 
LT.0.0: |NUMINT|  is  percentage  of  integration  points/layers 
which must fail before shell element fails.  For fully in-
tegrated  shells,  a  methodology  is  used  where  a  layer
fails  if  one  integration  point      fails  and  then  the  given
percentage  of  layers  must  fail  before  the  element  fails.
Only available for shells. 
Effective  plastic  strain  values  (optional  if  SIGY  is  defined).    At
least  2  points  should  be  defined.    The  first  point  must  be  zero
corresponding  to  the  initial  yield  stress.    WARNING:  If  the  first
point is nonzero the yield stress is extrapolated to determine the
initial  yield.    If  this  option  is  used  SIGY  and  ETAN  are  ignored
and may be input as zero. 
ES1 - ES8 
Corresponding yield stress values to EPS1 - EPS8. 
LCTSRF 
Load curve that defines the thinning strain at failure as a function
of the plastic strain rate.
*MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY 
DESCRIPTION
EPS0 
EPS0 parameter for RTCL damage. 
EQ.0.0: (default) RTCL damage is inactive. 
GT.0.0:  RTCL damage is active 
TRIAX 
RTCL damage triaxiality limit. 
EQ.0.0: (default) No limit. 
GT.0.0:  Damage  does  not  accumulate  when  triaxiality  exceeds
TRIAX. 
Remarks: 
Optional RTCL damage is used to fail elements when the damage function exceeds 1.0.  
During  each  solution  cycle,  if  the  plastic  strain  increment  is  greater  than  zero,  an 
increment of RTCL damage is calculated by 
𝛥𝑓damage =
𝜀0
𝑓 (
𝜎𝐻
𝜎̅̅̅̅̅
𝑑𝜀̅𝑝 
)
RTCL
where 
and, 
𝑓 (
𝜎𝐻
𝜎̅̅̅̅̅
)
=
RTCL
⎧0
{{
{{{{
{{
⎨
{{
{{{
{{{
⎩
1 +
𝜎𝐻
𝜎̅̅̅̅̅
𝜎𝐻
𝜎̅̅̅̅̅
√12 − 27(
+ √12 − 27(
1.65
exp (
3𝜎𝐻
2𝜎̅̅̅̅̅
)
𝜎𝐻
𝜎̅̅̅̅̅
𝜎𝐻
𝜎̅̅̅̅̅
𝜎𝐻
𝜎̅̅̅̅̅
≤ −
)
)
<
𝜎𝐻
𝜎̅̅̅̅̅
<
𝜎𝐻
𝜎̅̅̅̅̅
≥
𝜀0 = uniaxial fracture strain / critical damage value 
𝜎𝐻 = hydrostatic stress 
𝜎̅̅̅̅̅ = effective stress 
𝑑𝜀̅𝑝 = effective plastic strain increment 
The  increments  are  summed  through  time  and  the  element  is  deleted  when  𝑓damage ≥
1.0.  For 0.0 < 𝑓damage < 1.0,
 the element strength will not be degraded. 
The value of 𝑓damage is stored as history variable #9 and can be fringe plotted from d3plot 
files  if  the  number  of  extra  history  variables  requested  is  ≥  9  on  *DATABASE_EX-
TENT_BINARY.
The optional TRIAX parameter can be used to prevent excessive RTCL damage growth 
and  element  erosion  for  badly  shaped  elements  that  might  show  unrealistically  high 
values for the triaxiality.  The triaxiality, 
𝜎𝐻
𝜎̅̅̅̅̅ , is stored as history variable #11. 
The  EPSMAJ  parameter  is  compared  to  the  major  principal  strain  in  the  following 
senses: 
•  For  shells  it  is  the  maximum  eigenvalue  of  the  in-plane  strain  tensor  that  is 
incremented by the strain increments. 
•  For solid elements it is calculated as the maximum eigenvalue to the logarithmic 
strain tensor 
𝛆 =
ln(𝐅T𝐅), 
where  𝐅  is  the  global  deformation  gradient.    In  sum,  both  element  types  use  a 
natural strain measure for determining failure, the major strain calculated in this 
way is output as history variable #7. 
To get an idea about the probability of failure, an indicator 𝐷 is computed internally: 
𝐷 = max (
𝜀̅𝑝
FAIL
,
−𝜀3
EPSTHIN
,
𝜀𝐼
EPSMAJ
) 
and stored as history variable #10. 𝐷 ranges from 0 (intact) to 1 (failed). 𝜀̅𝑝, −𝜀3, and 𝜀𝐼 
are current values of effective plastic strain, thinning strain, and major in plane strain.  
This  instability  measure,  including  the  RTCL  damage,  can  also  be  retrieved  from 
requesting material histories 
*DEFINE_MATERIAL_HISTORIES Properties 
Label 
Attributes 
Description 
Instability 
Plastic Strain Rate 
- 
- 
- 
- 
- 
- 
- 
- 
Failure indicator max(𝐷, 𝑓damage) 
𝑝  
Effective plastic strain rate 𝜀̇eff
For  implicit  calculations  on  this  material  involving  severe  nonlinear  hardening  the 
radial return method may result in inaccurate stress-strain response.  Setting IACC = 1 
on *CONTROL_ACCURACY activates a fully iterative plasticity algorithm, which will 
remedy  this.    This  is  not  to  be  confused  with  the  MITER  flag  on  *CONTROL_SHELL, 
which governs the treatment of the plane  stress assumption for shell elements.   If any 
failure model is applied with this option, incident failure will initiate damage, and the 
stress will continuously degrade to zero before erosion for a deformation of 1% plastic 
strain.    So  for  instance,  if  the  failure  strain  is  FAIL = 0.05,  then  the  element  is  eroded 
when  𝜀̅𝑝 = 0.06  and  the  material  goes  from  intact  to  completely  damaged  between
𝜀̅𝑝 = 0.05 and 𝜀̅𝑝 = 0.06.  The reason is to enhance implicit performance by maintaining 
continuity in the internal forces.
*MAT_PLASTICITY_COMPRESSION_TENSION 
This  is  Material  Type  124.    An  isotropic  elastic-plastic  material  where  unique  yield 
stress  versus  plastic  strain  curves  can  be  defined  for  compression  and  tension.    Also, 
failure can occur based on a plastic strain or a minimum time step size.  Rate effects on 
the yield stress are modeled either by using the Cowper-Symonds strain rate model or 
by using two load curves that scale the yield stress values in compression and tension, 
respectively.   Material rate effects, which are independent of the  plasticity model, are 
based on a 6-term Prony series Maxwell mode that generates an additional stress tensor.  
The  viscous  stress  tensor  is  superimposed  on  the  stress  tensor  generated  by  the 
plasticity. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
Default 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
5 
C 
F 
0 
5 
6 
P 
F 
0 
6 
Variable 
LCIDC 
LCIDT 
LCSRC 
LCSRT 
SRFLAG 
LCFAIL 
Type 
Default 
  Card 3 
Variable 
Type 
Default 
I 
0 
1 
PC 
F 
0 
I 
0 
2 
PT 
F 
0 
I 
0 
3 
I 
0 
4 
F 
0 
5 
I 
0 
6 
PCUTC 
PCUTT 
PCUTF 
F 
0 
F 
0 
F 
0 
7 
8 
FAIL 
TDEL 
F 
10.E+20 
7 
EC 
F 
none 
7 
F 
0 
8 
RPCT 
F 
0
3 
4 
5 
6 
7 
8 
*MAT_124 
  Card 4 
Variable 
Type 
1 
K 
F 
Viscoelastic Constant Cards.  Up to 6 cards may be input.  A keyword card (with a 
“*” in column 1) terminates this input if less than 6 cards are used. 
  Card 5 
Variable 
Type 
1 
Gi 
F 
  VARIABLE   
MID 
RO 
E 
PR 
C 
P 
2 
3 
4 
5 
6 
7 
8 
BETAi 
F 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
Strain rate parameter, 𝐶, see formula below. 
Strain rate parameter, 𝑃, see formula below. 
FAIL 
Failure flag. 
LT.0.0:  User defined failure subroutine, matusr_24 in dyn21.F, 
is called to determine failure 
EQ.0.0:  Failure is not considered.  This option is recommended
if failure is not of interest since many calculations will
be saved. 
GT.0.0:  Plastic strain to failure.  When the plastic strain reaches
this value, the element is deleted from the calculation. 
TDEL 
Minimum time step size for automatic deletion of shell elements.
VARIABLE   
LCIDC 
LCIDT 
LCSRC 
LCSRT 
DESCRIPTION
Load  curve  ID  defining  effective  stress  versus  effective  plastic
strain  in  compression.    Enter  positive  yield  stress  and  plastic
strain values when defining this curve. 
Load  curve  ID  defining  effective  stress  versus  effective  plastic
strain  in  tension.    Enter  positive  yield  stress  and  plastic  strain
values when defining this curve. 
Optional load curve ID defining strain rate scaling factor on yield
stress versus strain rate when the material is in compression. 
Optional load curve ID defining strain rate scaling factor on yield
stress versus strain rate when the material is in tension. 
SRFLAG 
Formulation for rate effects: 
EQ.0.0:  Total strain rate, 
EQ.1.0:  Deviatoric strain rate.  
EQ.2.0:  Plastic strain rate (viscoplastic). 
LCFAIL 
EC 
RPCT 
PC 
PT 
Load  curve  ID  defining  failure  strain  versus  strain  rate.    See
Remarks for additional information. 
Optional Young’s modulus for compression, > 0. 
Fraction  of  PT  and  PC,  used  to  define  mean  stress  at  which
Young’s modulus is E and EC, respectively.  Young’s modulus is
E  when  mean  stress > RPCT ×  PT,  and  EC  when  mean  stress <  -
RPCT ×  PC.    If  the  mean  stress  falls  between  –RPCT ×  PC  and 
RPCT × PT, a linearly interpolated value is used. 
Compressive  mean  stress  (pressure)  at  which  the  yield  stress
follows  load  curve  ID,  LCIDC.    If  the  pressure  falls  between  PC
and PT a weighted average of the two load curves is used.  Both
PC and PT should be entered as positive values. 
Tensile  mean  stress  at  which  the  yield  stress  follows  load  curve
ID, LCIDT.
PCUTC 
*MAT_PLASTICITY_COMPRESSION_TENSION 
DESCRIPTION
Pressure cut-off in compression (PCUTC must be greater than or
equal to zero).  PCUTC (and PCUTT) apply only to element types
that use a 3D stress update, e.g., solids, tshell formulations 3 and 
5,  and  SPH.    When the  pressure  cut-off  is  reached  the  deviatoric 
stress  tensor  is  set  to  zero  and  the  pressure  remains  at  its
compressive  value.    Like  the  yield  stress,  PCUTC  is  scaled  to
account for rate effects. 
PCUTT 
Pressure cut-off in tension (PCUTT must be less than or equal to
zero).    When  the  pressure  cut-off  is  reached  the  deviatoric  stress 
tensor  and  tensile  pressure  is  set  to  zero.    Like  the  yield  stress,
PCUTT is scaled to account for rate effects. 
PCUTF 
Pressure cut-off flag activation. 
EQ.0.0:  Inactive, 
EQ.1.0:  Active. 
K 
Gi 
Optional bulk modulus for the viscoelastic material.  If nonzero a
Kelvin type behavior will be obtained.  Generally, 𝐾 is set to zero.
Optional shear relaxation modulus for the ith term 
BETAi 
Optional shear decay constant for the ith term 
Remarks: 
The  stress  strain  behavior  follows  a  different  curve  in  compression  than  it  does  in 
tension.    Tension  is  determined  by  the  sign  of  the  mean  stress  where  a  positive  mean 
stress  (i.e.,  a  negative  pressure)  is  indicative  of  tension.    Two  curves  must  be  defined 
giving  the  yield  stress  versus  effective  plastic  strain  for  both  the  tension  and 
compression regimes. 
Mean  stress  is  an  invariant  which  can  be  expressed  as  (𝜎𝑥 + 𝜎𝑦 + 𝜎𝑧)/3.    PC  and  PT 
define  a  range  of  mean  stress  values  within  which  interpolation  is  done  between  the 
tensile  yield  surface  and  compressive  yield  surface.      PC  and  PT  are  not  true  material 
properties  but  are  just  a  numerical  convenience  so  that  the  transition  from  one  yield 
surface to the other is not abrupt as the sign of the mean stress changes.  Both PC and 
PT  are  input  as  positive  values  as  it  is  implied  that  PC  is  a  compressive  mean  stress 
value and PT is tensile mean stress value. 
Strain  rate  may  be  accounted  for  using  the  Cowper  and  Symonds  model  which  scales 
the yield stress with the factor:
where 𝜀̇ is the strain rate, 
1 + [
𝑝⁄
𝜀̇
]
𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗. 
The LCFAIL field  is only applicable when at least one of the following four conditions 
are met: 
1.  SRFLAG = 2 
2.  LCSRC is nonzero 
3.  LCSRT is nonzero 
4.  Gi, BETAi values are provided.
*MAT_KINEMATIC_HARDENING_TRANSVERSELY_ANISOTROPIC_{OPTION} 
This  is  Material  Type  125.    This  material  model  combines  Yoshida  &  Uemori’s  non-
linear kinematic hardening rule with material type 37.  Yoshida & Uemori’s theory uses 
two surfaces to describe the hardening rule: the yield surface and the bounding surface.  
In the forming process, the yield surface does not change in size, but its center translates 
with deformation; the bounding surface changes both in size and location.  This model 
also  allows  the  change  of  Young’s  modulus  as  a  function  of  effective  plastic  strain  as 
proposed by Yoshida & Uemori [2002].  This material type is available for shells, thick 
shells and solid elements. 
Available options include: 
<BLANK> 
NLP 
The  NLP  option  estimates  necking  failure  using  the  Formability  Index  (F.I.),  which 
accounts  for  the  non-linear  strain  paths  seen  in  metal  forming  applications  .  Specify IFLD in card #3 when using this option, also see the example under 
the  remarks.    Since  the  NLP  option  also  works  under  linear  strain  path,  it  is 
recommended  to  be  used  as  the  default  failure  criterion  in  metal  forming.    The  NLP 
option is also available in *MAT_036, *MAT_037, and *MAT_226. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
R 
F 
I 
6 
7 
8 
HLCID 
OPT 
Default 
none 
none 
none 
none 
none 
none 
  Card 2 
Variable 
1 
CB 
Type 
F 
2 
Y 
F 
3 
SC1 
F 
4 
K 
F 
5 
RSAT 
F 
6 
SB 
F 
I 
0 
7 
H 
F 
8 
SC2 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
0.0
Card 3 
Variable 
1 
EA 
2 
3 
COE 
IOPT 
Type 
F 
F 
Default 
none 
none 
I 
0 
4 
C1 
F 
5 
C2 
F 
6 
7 
8 
IFLD 
I 
none 
none 
none 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
R 
HLCID 
OPT 
CB 
Y 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s Modulus 
Poisson’s ratio 
Anisotropic hardening parameter 
Load  curve  ID  in  keyword  *DEFINE_CURVE,  where  true  strain 
and true stress relationship is characterized.  This curve is used in
conjunction  with  variable  OPT,  and  not  to  be  referenced  or  used
in other keywords. 
The use of this parameter is not recommended. 
Error  calculation  flag.    When  OPT = 2,  LS-DYNA  will  perform 
error  calculation  based  on  the  true  stress-strain  curve  from 
uniaxial  tension,  specified  by  HLCID.    The  corrections  will  be
made to the cyclic load curve, both in the loading and unloading 
portions.    Since,  in  some  cases  where  loading  is  more  complex,
the accumulated plastic strain could be large (say more than 30%),
the  input  uniaxial  stress-strain  curve  must  have  enough  strain 
range  to  cover  the  maximum  expected  plastic  strain.    Note  this 
variable  must  be  set  to  a  value  of  “2”  if  HLCID  is  specified  and
stress-strain curve is used.  
The default value of “0” is recommended. 
The uppercase 𝐵 defined in Yoshida & Uemori’s equations. 
Hardening  parameter  appearing 
equations. 
in  Yoshida  &  Uemori’s
*MAT_KINEMATIC_HARDENING_TRANSVERSELY_ANISOTROPIC 
DESCRIPTION
SC1 
K 
RSAT 
SB 
H 
SC2 
EA 
COE 
The lowercase 𝑐 defined in the following equations, and 𝐶1 as in 
the remarks section. 
Hardening  parameter  appearing 
equations. 
in  Yoshida  &  Uemori’s
Hardening  parameter  appearing 
equations. 
in  Yoshida  &  Uemori’s 
The lowercase 𝑏 appearing in Yoshida & Uemori’s equations. 
Anisotropic  parameter 
stagnation. 
associated  with  work-hardening 
The lowercase 𝑐 defined in the following equations, and 𝐶2 as in
the remarks section.  If SC2 = 0.0, left blank, or SC2 = SC1, then it 
turns into the basic model. 
Variable  controlling  the  change  of  Young’s  modulus,  𝐸𝐴    in  the 
following equations. 
Variable  controlling  the  change  of  Young’s  modulus,  𝜁   in  the 
following equations. 
IOPT 
Modified kinematic hardening rule flag: 
EQ.0: Original Yoshida & Uemori formulation, 
EQ.1:  Modified formulation.  Define C1, C2 below. 
C1, C2 
Constants used to modify R: 
𝑅 = RSAT × [(𝐶1 + 𝜀̅𝑝)𝑐2 − 𝐶1
𝑐2] 
IFLD 
ID of a load curve defining Forming Limit Diagram (FLD) under
linear strain paths.  In the load curve, abscissas represent minor
strains  while  ordinates  represent  major  strains.    Define  only
when  the  option  NLP is  used.    See  the  example  in  the remarks 
section. 
The Yoshida & Uemori’s kinematic hardening model: 
According  to  F.    Yoshida  and  T.    Uemori’s  paper  titled  “A  model  of  large-strain  cyclic 
plasticity  describing  the  Bauschinger  effect  and  work  hardening  stagnation”  in  2002 
International Journal of Plasticity 18, 661-686, and referring to Figure M125-1,
𝛼∗ = 𝛼 − 𝛽 
𝛼∗ = 𝑐 [(
) (𝜎 − 𝛼) − √
𝛼∗
𝛼∗] 𝜀̅𝑝 
𝑎 = 𝐵 + 𝑅 − 𝑌 
The  change  of  size  and  location  for  the  bounding  surface  is  defined  as,  referring  to 
Figure M125-2, 
𝑅̇ = 𝑘(𝑅sat − 𝑅)𝜀̅
𝛽′
𝑏𝐷 − 𝛽′𝜀̅
= 𝑘(
̇𝑝, 
̇𝑝) 
In  Yoshida  &  Uemori’s  model,  there  is  work-hardening  stagnation  in  the  unloading 
process, and it is described as, 
𝜎bound = 𝐵 + 𝑅 + 𝛽 
𝑔𝜎(𝜎 ′, 𝑞′, 𝑟′) =
(𝜎 ′ − 𝑞′): (𝜎 ′ − 𝑞′) − 𝑟2 
𝑞′
= 𝜇(𝛽′ − 𝑞′) 
𝑟 = ℎΓ 
3(𝛽′ − 𝑞′): 𝛽′
2𝑟
Γ =
The change in Young’s modulus is defined as a function of effective strain, 
𝐸 = 𝐸0 − (𝐸0 − 𝐸𝐴)[1 − exp(−𝜁 𝜀̅𝑝)] 
Strain hardening saturation: 
in  NUMISHEET  2008  proceedings,  137-142,  2008, 
Further  improvements  in  the  original  Yoshida  &  Uemori’s  model,  as  described  in  a 
paper “Determination of Nonlinear Isotropic/Kinematic Hardening Constitutive Parameter for 
AHSS  using  Tension  and  Compression  Tests”,  by  Ming  F.    Shi,  Xinhai  Zhu,  Cedric  Xia, 
Thomas  Stoughton, 
included 
modifications to allow working hardening in large strain deformation region, avoiding 
the problem of earlier saturation, especially for Advanced High Strength Steel (AHSS).  
These types of steels exhibit continuous strain hardening behavior and a non-saturated 
isotropic hardening function.  As described in the paper, the evolution equation for R (a 
part of the current radius of the bounding surface in deviatoric stress space), as is with 
the  saturation  type  of  isotropic  hardening  rule  proposed  in  the  original  Yoshida  & 
Uemori model, 
𝑅̇ = 𝑚(𝑅sat − 𝑅)𝑝̇ 
is modified as,
𝑅 = RSAT × [(𝐶1 + 𝜀̅𝑝)𝑐2 − 𝐶1
𝑐2] 
For  saturation  type  of  isotropic  hardening  rule,  set  IOPT = 0,  applicable  to  most  of 
Aluminum sheet materials.  In addition, the paper provides detailed variables used for 
this  material  model  for  DDQ,  HSLA,  DP600,  DP780  and  DP980  materials.    Since  the 
symbols  used  in  the  paper  are  different  from  what  are  used  here,  the  following  table 
provides  a  reference  between  symbols  used  in  the  paper  and  variables  here  in  this 
keyword: 
B 
CB 
Y 
Y 
C 
SC1 
m 
K 
K 
Rsat 
b 
SB 
h 
H 
e0 
C1 
N 
C2 
Using the modified formulation and the material properties provided by the paper, the 
predicted  and  tested  results  compared  very  well  both  in  a  full  cycle  tension  and 
compression  test  and  in  a  pre-strained  tension  and  compression  test,  according  to  the 
paper. 
A Failure Criterion for Nonlinear Strain Paths (NLP): 
The NLP failure criterion and corresponding post processing procedures are described 
in  the  entries  for  *MAT_036  and  *MAT_037.    The  history  variables  for  every  element 
stored in d3plot files include: 
1.  Formability Index (F.I.): #1 
2.  Strain ratio (in-plane minor strain/major strain): #2 
3.  Effective strain from the planar isotropic assumption: #3 
The entire time history can be  plotted using Post/History menu in  LS-PrePost v4.0.  To 
enable  the  output  of  these  history  variables  to  the  d3plot  files,  NEIPS  on  the  *DATA-
BASE_EXTENT_BINARY card must be set to at least 3.  When plotting the formability 
index, first select the history var #1 from the Misc in the FriComp menu.  The pull-down 
menu  under  FriComp  can  be  used  to  select  minimum  value  ‘Min’  for  necking  failure 
determination  (refer  to  Tharrett  and  Stoughton’s  paper  in  2003  SAE  2003-01-1157).    In 
FriRang, the option None is to be selected in the pull-down menu next to Avg.  Lastly, set 
the  simulation  result  to  the  last  state  in  the animation  tool  bar.    The  index  value ranges 
from 0.0 to 1.5.  The non-linear forming limit is reached when the index reaches 1.0.
An Example of the NLP Option: 
A  partial  keyword  example  is  listed  below  when  the  option  NLP  is  used.    The 
traditional Forming Limit Diagram (FLD) which governs the linear strain paths only is 
defined by load curve ID 321. 
*MAT_KINEMATIC_HARDENING_TRANSVERSELY_ANISOTROPIC_NLP 
$#     mid        ro         e        pr         r     hclid       opt 
         1   7.83E-9   2.07E+5       0.3     1.035 
$#      cb         y        sc         k      rsat        sb         h 
     422.8     304.2     398.5      28.0     702.7     136.9      0.91 
$#      ea       coe      iopt        c1        c2      IFLD 
       0.0       0.0         1    0.0065     0.545       321 
*DEFINE_CURVE 
$ traditional FLD data (major vs.  minor) 
321 
-0.357,0.596 
⋮ 
⋮ 
-0.020,0.260 
 0.000,0.239 
 0.010,0.244 
 0.020,0.249 
⋮ 
⋮ 
 0.239,0.354 
 0.247,0.356 
 0.262,0.361 
 0.372,0.361 
*END 
Application results: 
Application  of  the  modified  Yoshida  &  Uemori’s  hardening  rule  in  the  metal  forming 
industry has shown significant advantage in springback prediction accuracy, especially 
for  AHSS  type  of  sheet  materials.    As  shown  in  Figure  M125-3  (left),  predicted 
springback shape of an automotive shotgun (also called: upper load path/beam) using 
*MAT_125  is  compared  with  experimental  measurements  on  a  DP780  material.  
Prediction accuracy achieved over 92% with *MAT_125 while about 61% correlation is 
found with *MAT_037 (Figure M125-3 right), a remarkable improvement. 
In another example, NUMISHEET 2011 BM4 is used to demonstrate the application of 
the  Young’s  modulus  variations  as  a  function  of  effective  strain  in  prediction  of 
springback.  The sheet blank is a DP780 material with an initial thickness of 1.4mm.  The 
simulation  process  is  shown  (Figure  M125-4)  as  pre-straining  (to  8%),  springback, 
trimming, forming and springback.  Young’s modulus variations with effective strains 
are  accounted  for  by  curve  fitting  the  provided  experimental  data  to  obtain  the 
variables EA and COE, Figure M125-5.  Referring to Figures M125-6 and M125-7, final 
springback  shapes  of  the  cross  sectional  view  are  compared  with  measurement 
provided,  along  with  benchmark  results  from  software  X  and  Y.    In  addition, 
springback with no pre-straining is also conducted and correlated, shown in the same 
figures.    Furthermore,  hysteretic  plasticity  with  a  full  cycle  tension  and  compression 
simulation  is  done  on  one  single  shell  element  and  the  result  is  superimposed  with 
experimental date, in Figure M125-8.
To  improve  convergence  and  for  a  faster  simulation  time,  it  is  recommended  that 
*CONTROL_IMPLICIT_FORMING  type  ‘1’  be  used  when  conducting  a  springback 
simulation. 
About SC1 and SC2: 
In  F.    Yoshida  and  T.    Uemori’s  2002  paper,  the  effect  of  variables  SC1  and  SC2  were 
discussed.    According  to  the  paper,  variables  SC1  and  SC2  are  used  to  describe  the 
forward and reverse deformations of the cyclic plasticity curve, respectively.  It allows 
for  a  more  rapid  change  of  work  hardening  rate  in  the  vicinity  of  the  initial  yielding 
(~0.5% equivalent plastic strain), in the form of the following equations: 
SC =
⎧
{{
⎨
{{
⎩
SC1
max(𝛼̅∗) < 𝐵 − 𝑌
SC2
otherwise
where max(𝛼̅∗) is the maximum value of 𝛼̅∗, and, 
𝛼̅∗ = √
𝛼∗: 𝛼∗ 
As  shown  in  Figure  M125-9  from  Yoshida  &  Uemori’s  original  paper,  the  effect  of  a 
curve fitting is shown for a high strength steel (SPFC) using both SC1 and SC2, which 
fits much better than the fitting using only SC1.  In addition, in Figure M125-10, a much 
better  fitting  is  demonstrated  with  SC1  and  SC2  than  with  SC1  only  for  a  DP980 
material. 
Inclusion of shell normal stress: 
When  *LOAD_SURFACE_STRESS  is  used  in  the  input  deck  together  with  *MAT_125, 
normal  stresses  (either  from  sliding  contact  or  applied  pressure)  are  accounted  for 
during  the  simulation.    The  negative  local  𝑧-stresses  (select  z-stress  under  FCOMP  → 
Stress  and  select  local  under  FCOMP  in  LS-PrePost)  caused  by  the  sliding  contact  or 
applied  pressure  can  be  viewed  from  d3plot  files  after  Revision  97158.    It  is  found  in 
some cases this inclusion can improve forming simulation accuracy. 
Revision information: 
The variables HLCID, OPT, IOPT, C1, and C2 are available starting in Revision 46217.  
The variables SC1 and SC2 are available starting in Revision 74884.  The option NLP is 
available  in  explicit  dynamic  analysis  starting  in  Revision  95594.    Normal  stresses 
inclusion  is  available  starting  in  Revision  97158.    Later  Revisions  include  various 
improvements and should be used.
Bounding surface
Dp
Yield surface
*
B+R
Figure M125-1.  Schematic illustration of the two-surface model is the original 
center of the yield surface, 𝛼∗ is the current center for the yield surface; 𝛼 is the 
center of the bounding surface. 𝛽 represents the relative position of the centers 
of  the  two  surfaces.    Y  is  the  size  of  the  yield  surface  and  is  constant
throughout the deformation process.  B+R represents the size of the bounding
surface, with R being associated with isotropic hardening. Reproduced from the 
original Yoshida and Uemori’s paper. 
Bounding surface F
β'
q'
gσ 
gσ 
β'
q'o
β'
q'
(a) when R = 0
(b) when R > 0
Figure  M125-2.    Change  in  bounding  surface  (reproduced  from  the  original 
Yoshida and Uemori’s paper).
Red:      measured
Black:  simulation
92.51% of sampled points 
within 1mm deviation
61.78% of sampled points 
within 1mm deviation
Max. 6.63mm
Max. 2.42mm
*MAT_125
*MAT_037
Figure M125-3.  Comparison of springback prediction on the A/S P load beam
(reproduced from an original color contour map courtesy of Chrysler LLC and United
States Steel Corporation).
Blanking
Pre-straining
Springback
Trimming
Forming
Forming complete
Springback
  Figure M125-4.  NUMISHEET 2011 Benchmark #4 simulation procedure. 
)
(
'
200
195
190
185
180
175
 170
 165
Young's Modulus Evolution
Fitted for LS-DYNA
Test
0.02
0.04
0.06
0.08
0.10
0.12
Equivalent plastic strain
Figure M125-5.  Curve fitting with coefficients: EA = 1.668E+05; COE = 95.0.
Springback Profile: No Prestrain
Springback Profile: 8% Prestrain
 70
 60
 50
 40
 30
 20
 10
 0
Test
LS-DYNA
Software X
 0
 20
 40
 60
 80
 100
 120
 140
mm
 70
 60
 50
 40
 30
 20
 10
 0
Test
LS-DYNA
Software X
 0
 20
 40
 60
mm
 80
 100
 120
Figure M125-6.  Comparison of springback profile with software X:  0% (left)
and 8% prestrain (right) 
Springback Profile: No Prestrain
Springback Profile: 8% Prestrain
 70
 60
 50
 40
 30
 20
 10
 0
Test
LS-DYNA
Software Y
 0
 20
 40
 60
 80
 100
 120
 140
mm
 70
 60
 50
 40
 30
 20
 10
 0
Test
LS-DYNA
Software Y
 0
 20
 40
 60
mm
 80
 100
 120
Figure M125-7.  Comparison of springback profile with software Y:  0% (left)
and 8% prestrain(right) 
Uni-axial tension
Uni-axial tension
Cyclic test
M125 result
)
(
800
400
-400
-800
Unstrained
Uni-axial compression
0.04
0.08
True strain
Figure M125-8.  Cyclic plasticity verification on one element.
)
(
800
700
600
500
400
300
200
100
Experiment
Basic model(SC1=200)
Modified model (SC1=2000, SC2=200 in Eq. (1)
0.01
0.02
0.03
0.04
0.05
0.06
True strain 
Figure M125-9.  Effect of SC1 and SC2 (reproduced from the original Yoshida & 
Uemori’s paper).
1200
900
600
300
-300
-600
-900
-1200
1200
900
600
300
-300
-600
-900
-1200
Experimental result
Curve fitting result
SC1 + SC2
-0.03
0.03
SC1 only
-0.03
0.03
Figure M125-10.  Material curve fitting comparison (reproduced from an original
color slide   courtesy of CYBERNET SYSTEMS CO., LTD.).
*MAT_MODIFIED_HONEYCOMB 
This  is  Material  Type  126.    The  major  use  of  this  material  model  is  for  aluminum 
honeycomb  crushable  foam  materials  with  anisotropic  behavior.    Three  yield  surfaces 
are  available.    In  the  first,  nonlinear  elastoplastic  material  behavior  can  be  defined 
separately  for  all  normal  and  shear  stresses,  which  are  considered  to  be  fully 
uncoupled.  In the second, a yield surface is defined that considers the effects of off-axis 
loading.  The second yield surface is transversely isotropic.  A drawback of this second 
yield  surface  is  that  the  material  can  collapse  in  a  shear  mode  due  to  low  shear 
resistance.    There  was  no  obvious  way  of  increasing  the  shear  resistance  without 
changing  the  behavior  in  purely  uniaxial  compression.    Therefore,  in  the  third  option, 
the  model  has  been  modified  so  that  the  user  can  prescribe  the  shear  and  hydrostatic 
resistance  in  the  material  without  affecting  the  uniaxial  behavior.    The  choice  of  the 
second  yield  surface  is  flagged  by  the  sign  of  the  first  load  curve  ID,  LCA.    The  third 
yield surface is flagged by the sign of ECCU, which becomes the initial stress yield limit 
in simple shear.  A description is given below. 
The development of the second and third yield surfaces are based on experimental test 
results of aluminum honeycomb specimens at Toyota Motor Corporation. 
The  default  element  for  this  material  is  solid  type  0,  a  nonlinear  spring  type  brick 
element.  The recommended hourglass control is the type 2 viscous formulation for one 
point integrated solid elements.  The stiffness form of the hourglass control when used 
with this constitutive model can lead to nonphysical results since strain localization in 
the shear modes can be inhibited. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
SIGY 
F 
6 
VF 
F 
7 
8 
MU 
BULK 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
.05 
0.0
Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCA 
LCB 
LCC 
LCS 
LCAB 
LCBC 
LCCA 
LCSR 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
LCA 
LCA 
LCA 
LCS 
LCS 
LCS 
optional
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EAAU 
EBBU 
ECCU 
GABU 
GBCU 
GCAU 
AOPT 
MACF 
Type 
F 
F 
F 
F 
F 
F 
  Card 4 
Variable 
1 
XP 
Type 
F 
  Card 5 
Variable 
1 
D1 
Type 
F 
2 
YP 
F 
2 
D2 
F 
3 
ZP 
F 
3 
D3 
F 
4 
A1 
F 
4 
5 
A2 
F 
5 
6 
A3 
F 
6 
I 
8 
7 
7 
8 
TSEF 
SSEF 
VREF 
TREF 
SHDFLG 
F 
F 
F 
F 
F 
Additional card for AOPT = 3 or AOPT = 4. 
  Card 6 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
5 
6 
7
*MAT_MODIFIED_HONEYCOMB 
  Card 7 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCSRA 
LCSRB 
LCSRC 
LCSRAB 
LCSRBC 
LCSCA 
Type 
F 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
SIGY 
VF 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus for compacted honeycomb material. 
Poisson’s ratio for compacted honeycomb material. 
Yield stress for fully compacted honeycomb. 
Relative  volume  at  which  the  honeycomb  is  fully  compacted.
This parameter is ignored for corotational solid elements, types 0
and 9. 
MU 
μ, material viscosity coefficient.  (default=.05)  Recommended. 
BULK 
Bulk viscosity flag: 
EQ.0.0: bulk viscosity is not used.  This is recommended. 
EQ.1.0: bulk viscosity is active and μ = 0.  This will give results 
identical to previous versions of LS-DYNA. 
LCA 
Load curve ID, see *DEFINE_CURVE: 
LCA.LT.0:  Yield  stress  as  a  function  of  the  angle  off  the 
material axis in degrees.   
LCA.GT.0: sigma-aa  versus  normal  strain  component  aa.    For 
the corotational solid elements, types 0 and 9, engi-
neering strain is expected, but for all other solid el-
ement formulations a logarithmic strain is expected.
See Remarks.
VARIABLE   
DESCRIPTION
LCB 
Load curve ID, see *DEFINE_CURVE: 
LCA.LT.0:  strong  axis  hardening  stress  as  a  function  of  the
volumetric strain.   
LCA.GT.0: sigma-bb  versus  normal  strain  component  bb.    For 
the corotational solid elements, types 0 and 9, engi-
neering strain is expected, but for all other solid el-
ement formulations a logarithmic strain is expected.
Default LCB = LCA.  See Remarks. 
LCC 
Load curve ID, see *DEFINE_CURVE: 
LCA.LT.0:  weak  axis  hardening  stress  as  a  function  of  the
volumetric strain. 
LCA.GT.0: sigma-cc  versus  normal  strain  component  cc.    For 
the corotational solid elements, types 0 and 9, engi-
neering strain is expected, but for all other solid el-
ement formulations a logarithmic strain is expected.
Default LCC = LCA.  See Remarks. 
LCS 
Load curve ID, see *DEFINE_CURVE: 
LCA.LT.0:  damage  curve  giving  shear  stress  multiplier  as  a
function  of  the  shear  strain  component.    This  curve
definition is optional and may be used if damage is
desired.    IF  SHDFLG = 0  (the  default),  the  damage 
value  multiplies  the  stress  every  time  step  and  the
stress is updated incrementally.  The damage curve
should  be  set  to  unity  until  failure  begins.   After 
failure the value should drop to 0.999 or 0.99 or any
number  between  zero  and  one  depending  on  how
many  steps  are  needed  to  zero  the  stress.    Alterna-
tively,  if  SHDFLG = 1,  the  damage  value  is  treated 
as  a  factor  that  scales  the  shear  stress  compared  to
the undamaged value. 
LCA.GT.0: shear stress versus shear strain.  For the corotational
solid  elements,  types  0  and  9,  engineering  strain  is
expected,  but  for  all  other  solid  element  formula-
tions a shear strain based on the deformed configu-
  Each 
ration 
component  of  shear  stress  may  have  its  own  load
curve.  See Remarks. 
  Default  LCS = LCA. 
is  used.
*MAT_MODIFIED_HONEYCOMB 
DESCRIPTION
LCAB 
Load curve ID, see *DEFINE_CURVE.  Default LCAB = LCS: 
LCA.LT.0:  damage curve giving shear ab-stress multiplier as a 
function  of  the  ab-shear  strain  component.    This 
curve  definition  is  optional  and  may  be  used  if
damage is desired.  See LCS above. 
LCA.GT.0: sigma-ab versus shear strain-ab.  For the corotation-
al solid elements, types 0 and 9, engineering strain is
expected,  but  for  all  other  solid  element  formula-
tions a shear strain based on the deformed configu-
ration is used.  See Remarks. 
LCBC 
Load curve ID, see *DEFINE_CURVE.  Default LCBC = LCS: 
LCA.LT.0:  damage curve giving bc-shear stress multiplier as a 
function  of  the  ab-shear  strain  component.    This 
curve  definition  is  optional  and  may  be  used  if
damage is desired.  See LCS above. 
LCA.GT.0: sigma-bc versus shear strain-bc.  For the corotation-
al solid elements, types 0 and 9, engineering strain is
expected,  but  for  all  other  solid  element  formula-
tions a shear strain based on the deformed configu-
ration is used.  See Remarks. 
LCCA 
Load curve ID, see *DEFINE_CURVE.  Default LCCA = LCS: 
LCA.LT.0:  damage curve giving ca-shear  stress multiplier as a 
function  of  the  ca-shear  strain  component.    This 
curve  definition  is  optional  and  may  be  used  if
damage is desired.  See LCS above. 
LCA.GT.0: sigma-ca versus shear strain-ca.  For the corotational 
solid  elements,  types  0  and  9,  engineering  strain  is
expected,  but  for  all  other  solid  element  formula-
tions a shear strain based on the deformed configu-
ration is used.  See Remarks. 
LCSR 
the 
Load  curve  ID,  see  *DEFINE_CURVE,  for  strain-rate  effects 
defining 
rate
factor  versus 
𝑖𝑗𝜀′̇
3 (𝜀′̇
̇ = √2
scaled using this curve. 
𝑖𝑗).    This  is  optional.    The  curves  defined  above  are
effective 
strain 
scale 
𝜀̅
EAAU 
Elastic modulus Eaau in uncompressed configuration.
VARIABLE   
DESCRIPTION
EBBU 
ECCU 
GABU 
GBCU 
GCAU 
Elastic modulus Ebbu in uncompressed configuration. 
Elastic modulus Eccu in uncompressed configuration. 
LT.0.0: 𝜎𝑑
𝑌,  |ECCU|  initial  stress  limit  (yield)  in  simple  shear.
Also,  LCA < 0  to  activate  the  transversely  isotropic 
yield surface. 
Shear modulus Gabu in uncompressed configuration. 
Shear modulus Gbcu in uncompressed configuration. 
Shear modulus Gcau in uncompressed configuration. 
ECCU.LT.0.0: 𝜎𝑝
𝑌,  GCAU 
initial  stress 
in 
hydrostatic  compression.    Also,  LCA < 0  to  acti-
vate the transversely isotropic yield surface. 
(yield) 
limit 
AOPT 
Material  axes  option  : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES. 
EQ.1.0: locally orthotropic with material axes determined by a
point  in  space  and  the  global  location  of  the  element
center; this is the a-direction. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the
element  normal.    The  plane  of  a  solid  element  is  the 
midsurface between the inner surface and outer surface
defined by the first four nodes and the last four nodes
of the connectivity of the element, respectively. 
EQ.4.0: locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector  v,  and 
an originating point, p, which define the centerline ax-
is.  This option is for solid elements only.
*MAT_MODIFIED_HONEYCOMB 
DESCRIPTION
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).   
MACF 
Material axes change flag: 
EQ.1: No change, default, 
EQ.2: switch material axes a and b, 
EQ.3: switch material axes a and c, 
EQ.4: switch material axes b and c. 
XP YP ZP 
Coordinates of point p for AOPT = 1 and 4. 
A1 A2 A3 
Components of vector a for AOPT = 2. 
D1 D2 D3 
Components of vector d for AOPT = 2. 
V1 V2 V3 
Define components of vector v for AOPT = 3 and 4. 
TSEF 
SSEF 
2-680 (EOS) 
Tensile strain at element failure (element will erode).
VARIABLE   
VREF 
TREF 
DESCRIPTION
This is an optional input parameter for solid elements types 1, 2,
3, 4, and 10.  Relative volume at which the reference geometry is
stored.  At this time the element behaves like a nonlinear spring.
The TREF, below, is reached first then VREF will have no effect. 
This is an optional input parameter for solid elements types 1, 2,
3,  4,  and  10.    Element  time  step  size  at  which  the  reference
geometry  is  stored.    When  this  time  step  size  is  reached  the
element  behaves  like  a  nonlinear  spring.    If  VREF,  above,  is
reached first then TREF will have no effect. 
SHDFLG 
Flag  defining  treatment  of  damage  from  curves  LCS,  LCAB,
LCBC and LCCA (relevant only when LCA < 0): 
LCSRA 
EQ.0.0: Damage reduces shear stress every time step, 
EQ.1.0: Damage = (shear stress)/(undamaged shear stress) 
Optional  load  curve  ID  if  LCSR = -1,  see  *DEFINE_CURVE,  for 
strain  rate  effects  defining  the  scale  factor  for  the  yield  stress  in
the a-direction versus the natural logarithm of the absolute value 
of deviatoric strain rate in the a-direction.  This curve is optional. 
The scale factor for the lowest value of strain rate defined by the
curve  is  used  if  the  strain  rate  is  zero.    The  scale  factor  for  the
highest value of strain rate defined by the curve also defines the
upper limit of the scale factor. 
LCSRB 
Optional  load  curve  ID  if  LCSR = -1,  see  *DEFINE_CURVE,  for 
strain  rate  effects  defining  the  scale  factor  for  the  yield  stress  in
the b-direction versus the natural logarithm of the absolute value 
of deviatoric strain 
LCSRC 
Similar definition as for LCSA and LCSB above. 
LCSRAB 
Similar definition as for LCSA and LCSB above. 
LCSRBC 
Similar definition as for LCSA and LCSB above. 
LCSRCA 
Similar definition as for LCSA and LCSB above. 
Remarks: 
For  efficiency  it  is  strongly  recommended  that  the  load  curve  ID’s:  LCA,  LCB,  LCC, 
LCS,  LCAB,  LCBC,  and  LCCA,  contain  exactly  the  same  number  of  points  with 
corresponding  strain  values  on  the  abscissa.    If  this  recommendation  is  followed  the
cost  of  the  table  lookup  is  insignificant.    Conversely,  the  cost  increases  significantly  if 
the abscissa strain values are not consistent between load curves. 
For  solid  element  formulations  1  and  2,  the  behavior  before  compaction  is  orthotropic 
where the components of the stress tensor are uncoupled, i.e., an a component of strain 
will  generate  resistance  in  the  local  a-direction  with  no  coupling  to  the  local  b  and  c 
directions.    The  elastic  moduli  vary  from  their  initial  values  to  the  fully  compacted 
values linearly with the relative volume: 
𝐸𝑎𝑎 = 𝐸𝑎𝑎𝑢 + 𝛽(𝐸 − 𝐸𝑎𝑎𝑢)
𝐸𝑏𝑏 = 𝐸𝑏𝑏𝑢 + 𝛽(𝐸 − 𝐸𝑏𝑏𝑢) 
𝐸𝑐𝑐 = 𝐸𝑐𝑐𝑢 + 𝛽(𝐸 − 𝐸𝑐𝑐𝑢)
𝐺𝑎𝑏 = 𝐸𝑎𝑏𝑢 + 𝛽(𝐺 − 𝐺𝑎𝑏𝑢)
𝐺𝑏𝑐 = 𝐺𝑏𝑐𝑢 + 𝛽(𝐺 − 𝐺𝑏𝑐𝑢) 
𝐺𝑐𝑎 = 𝐺𝑐𝑎𝑢 + 𝛽(𝐺 − 𝐺𝑐𝑎𝑢)
where 
𝛽 = max [min (
1 − 𝑉
1 − 𝑉𝑓
, 1) , 0] 
and G is the elastic shear modulus for the fully compacted honeycomb material 
𝐺 =
2(1 + 𝑣)
The  relative  volume,  V,  is  defined  as  the  ratio  of  the  current  volume  over  the  initial 
volume, and typically, V = 1 at the beginning of a calculation.  
For  corotational  solid  elements,  types  0  and  9,  the  components  of  the  stress  tensor 
remain  uncoupled  and  the  uncompressed  elastic  moduli  are  used,  that  is,  the  fully 
compacted elastic moduli are ignored. 
The  load  curves  define  the  magnitude  of  the  stress  as  the  material  undergoes 
deformation.    The  first  value  in  the  curve  should  be  less  than  or  equal  to  zero 
corresponding to tension and increase to full compaction.  Care should be taken when 
defining the curves so the extrapolated values do not lead to negative yield stresses. 
At  the  beginning  of  the  stress  update  we  transform  each  element’s  stresses  and  strain 
rates into the local element coordinate system.  For the uncompacted material, the trial 
stress components are updated using the elastic interpolated moduli according to: 
𝑛+1trial
𝜎𝑎𝑎
= 𝜎𝑎𝑎
𝑛 + 𝐸𝑎𝑎Δ𝜀𝑎𝑎
𝑛+1trial
𝜎𝑐𝑐
𝑛+1trial
𝜎𝑏𝑏
= 𝜎𝑐𝑐
= 𝜎𝑏𝑏
𝑛 + 𝐸𝑐𝑐Δ𝜀𝑐𝑐 
𝑛 + 𝐸𝑏𝑏Δ𝜀𝑏𝑏
𝑛+1trial
𝜎𝑎𝑏
𝑛+1trial
𝜎𝑏𝑐
= 𝜎𝑎𝑏
𝑛 + 2𝐺𝑎𝑏Δ𝜀𝑎𝑏 
= 𝜎𝑏𝑐
𝑛 + 2𝐺𝑏𝑐Δ𝜀𝑏𝑐 
𝑛+1trial
𝜎𝑐𝑎
= 𝜎𝑐𝑎
𝑛 + 2𝐺𝑐𝑎Δ𝜀𝑐𝑎 
If  LCA > 0,  each  component  of  the  updated  stress  tensor  is  checked  to  ensure  that  it 
does not exceed the permissible value determined from the load curves, e.g., if
then 
𝑛+1trial
∣𝜎𝑖𝑗
∣ > 𝜆𝜎𝑖𝑗(𝜀𝑖𝑗) 
𝑛+1 = 𝜎𝑖𝑗(𝜀𝑖𝑗)
𝜎𝑖𝑗
𝑛+1trial
𝜆𝜎𝑖𝑗
𝑛+1trial∣
∣𝜎𝑖𝑗
On  Card  3 𝜎𝑖𝑗(𝜀𝑖𝑗)  is  defined  in  the  load  curve  specified  in  columns  31-40  for  the  aa 
stress component, 41-50 for the bb component, 51-60 for the cc component, and 61-70 for 
the ab, bc, cb shear stress components.  The parameter λ is either unity or a value taken 
from  the  load  curve  number,  LCSR,  that  defines  λ as  a  function  of  strain-rate.    Strain-
rate is defined here as the Euclidean norm of the deviatoric strain-rate tensor. 
If  LCA < 0,  a  transversely  isotropic  yield  surface  is  obtained  where  the  uniaxial  limit 
stress,  𝜎 𝑦(𝜑, 𝜀vol),  can  be  defined  as  a  function  of  angle  𝜑  with  the  strong  axis  and 
volumetric  strain,  𝜀vol.    In  order  to  facilitate  the  input  of  data  to  such  a  limit  stress 
surface, the limit stress is written as: 
𝜎 𝑦(𝜑, 𝜀vol) = 𝜎 𝑏(𝜑) + (cos𝜑)2𝜎 𝑠(𝜀vol) + (sin𝜑)2𝜎 𝑤(𝜀vol) 
where  the  functions  𝜎 𝑏,  𝜎 𝑠,  and  𝜎 𝑤  are  represented  by  load  curves  LCA,  LCB,  LCC, 
respectively.  The latter two curves can be used to include the stiffening effects that are 
observed  as  the  foam  material  crushes  to  the  point  where  it  begins  to  lock  up.      To 
ensure that the limit stress decreases with respect to the off-angle the curves should be 
defined such that following equations hold: 
and  
∂𝜎 𝑏(𝜑)
∂𝜑
≤ 0 
𝜎 𝑠(𝜀vol) − 𝜎 𝑤(𝜀vol) ≥ 0. 
A drawback of this implementation was that the material often collapsed in shear mode 
due  to  low  shear  resistance.    There  was  no  way  of  increasing  the  shear  resistance 
without  changing  the  behavior  in  pure  uniaxial  compression.    We  have  therefore 
modified the model so that the user can optionally prescribe the shear and hydrostatic 
resistance  in  the  material  without  affecting  the  uniaxial  behavior.      We  introduce  the 
𝑌(𝜀vol) as the hydrostatic and shear limit stresses, respectively.  
parameters 𝜎𝑝
These are functions of the volumetric strain and are assumed given by  
𝑌(𝜀vol) and 𝜎𝑑
𝑌(𝜀vol) = 𝜎𝑝
𝜎𝑝
𝑌(𝜀vol) = 𝜎𝑑
𝜎𝑑
𝑌 + 𝜎 𝑠(𝜀vol)
, 
𝑌 + 𝜎 𝑠(𝜀vol)
where we have reused the densification function 𝜎 𝑠. The new parameters are the initial 
𝑌,  and  are  provided by  the  user  as 
hydrostatic  and  shear  limit  stress  values,  𝜎𝑝
GCAU  and  |ECCU|,  respectively.    The  negative  sign  of  ECCU  flags  the  third  yield 
𝑌  and  𝜎𝑑
𝑌(𝜀vol)  and  (iii)  for  a  simple  shear  the  stress  limit  is  given  by  𝜎𝑑
surface  option  whenever  LCA < 0.    The  effect  of  the  third  formulation  is  that  (i)  for  a 
uniaxial stress the stress limit is given by 𝜎 𝑌(𝜙, 𝜀vol), (ii) for a pressure the stress limit is 
𝑌(𝜀vol).   
given  by  𝜎𝑝
Experiments have shown that the model may give noisy responses and inhomogeneous 
deformation modes if parameters are not chosen with care.  We therefore recommend to 
(i)  avoid  large  slopes  in  the  function  𝜎 𝑃,  (ii)  let  the  functions  𝜎 𝑠  and  𝜎 𝑤  be  slightly 
increasing  and  (iii)  avoid  large  differences  between  the  stress  limit  values  𝜎 𝑦(𝜑, 𝜀vol), 
𝑌(𝜀vol).  These  guidelines  are  likely  to  contradict  how  one  would 
𝑌(𝜀vol)  and  𝜎𝑑
𝜎𝑝
interpret  test  data  and  it  is  up  to  the  user  to  find  a  reasonable  trade-off  between 
matching experimental results and avoiding the mentioned numerical side effects. 
For  fully  compacted  material  (element  formulations  1  and  2),  we  assume  that  the 
material  behavior  is  elastic-perfectly  plastic  and  updated  the  stress  components 
according to: 
trial = 𝑠𝑖𝑗
𝑠𝑖𝑗
𝑛 + 2𝐺Δ𝜀𝑖𝑗
𝑑𝑒𝑣𝑛+1
2⁄
where the deviatoric strain increment is defined as 
Δ𝜀𝑖𝑗
𝑑𝑒𝑣 = Δ𝜀𝑖𝑗 −
Δ𝜀𝑘𝑘𝛿𝑖𝑗. 
We now check to see if the yield stress for the fully compacted material is exceeded by 
comparing  
trial = (
𝑠eff
2⁄
trial)
trial𝑠𝑖𝑗
𝑠𝑖𝑗
the effective trial stress to the yield stress, σy (Card 1, field  41-50).  If the effective trial 
stress exceeds the yield stress we simply scale back the stress components to the yield 
surface 
We can now update the pressure using the elastic bulk modulus, K 
𝑛+1 =
𝑠𝑖𝑗
𝜎𝑦
trial
𝑠eff
trial. 
𝑠𝑖𝑗
𝑛+1
𝑝𝑛+1 = 𝑝𝑛 − 𝐾Δ𝜀𝑘𝑘
2⁄
𝐾 =
3(1 − 2𝑣)
and obtain the final value for the Cauchy stress 
𝑛+1 = 𝑠𝑖𝑗
𝜎𝑖𝑗
𝑛+1 − 𝑝𝑛+1𝛿𝑖𝑗 
After  completing  the  stress  update  we  transform  the  stresses  back  to  the  global 
configuration.
For  *CONSTRAINED_TIED_NODES_WITH_FAILURE,  the  failure  is  based  on  the 
volume strain instead to the plastic strain. 
Curve extends into negative strain 
quadrant since LS-DYNA will 
extrapolate using the two end points.
It is important that the extropolation 
does not extend into the negative 
stress region.
 σ
ij
unloading and
reloading path
Strain: -ε
ij
Unloading is based on the interpolated Young’s 
moduli which must provide an unloading tangent 
that exceeds the loading tangent.
Figure M126-1.  Stress versus strain.  Note that the “yield stress” at a strain of
zero is nonzero.  In the load curve definition the “time” value is the directional
strain and the “function” value is the yield stress.   Note that for element types
0 and  9 engineering strains are  used, but for all other element types  the rates
are integrated in time.
*MAT_ARRUDA_BOYCE_RUBBER 
This is Material Type 127.  This material model provides a hyperelastic rubber model, 
see [Arruda and Boyce 1993] combined optionally with linear viscoelasticity as outlined 
by [Christensen 1980]. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
K 
F 
3 
Variable 
LCID 
TRAMP 
NT 
Type 
F 
F 
F 
4 
G 
F 
4 
5 
N 
F 
5 
6 
7 
8 
6 
7 
8 
Viscoelastic Constant Cards.  Up to 6 cards may be input.  A keyword card (with a 
“*” in column 1) terminates this input if less than 6 cards are used.  
  Card 3 
Variable 
Type 
1 
GI 
F 
  VARIABLE   
MID 
2 
3 
4 
5 
6 
7 
8 
BETAI 
F 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density 
K 
G 
N 
Bulk modulus 
Shear modulus 
Number of statistical links
VARIABLE   
LCID 
DESCRIPTION
Optional  load  curve  ID  of  relaxation  curve  if  constants  βI  are 
determined via a least squares fit.  This relaxation curve is shown
in Figure M76-1.  This model ignores the constant stress. 
TRAMP 
Optional ramp time for loading. 
NT 
Number of Prony series terms in optional fit.  If zero, the default
is  6.    Currently,  the  maximum  number  is  6.    Values  less  than  6,
possibly  3-5  are  recommended,  since  each  term  used  adds 
significantly  to  the  cost.    Caution  should  be  exercised  when
taking the results from the fit.  Always check the results of the fit
in the output file.  Preferably, all generated coefficients should be
positive.    Negative  values  may  lead  to  unstable  results.    Once  a 
satisfactory  fit  has  been  achieved  it  is  recommended  that  the
coefficients  which  are  written  into  the  output  file  be  input  in
future runs. 
GI 
Optional shear relaxation modulus for the ith term. 
BETAI 
Optional decay constant if ith term. 
Remarks: 
Rubber  is  generally  considered  to  be  fully  incompressible  since  the  bulk  modulus 
greatly  exceeds  the  shear  modulus  in  magnitude.    To  model  the  rubber  as  an 
unconstrained material a hydrostatic work term, 𝑊𝐻(𝐽), is included in the strain energy 
functional which is function of the relative volume, J, [Ogden 1984]: 
𝑊(𝐽1, 𝐽2, 𝐽) = 𝑛𝑘𝜃 [
(𝐽1 − 3) +
20𝑁
2 − 9) +
(𝐽1
+ 𝑛𝑘𝜃 [
19
7000𝑁3 (𝐽1
4 − 81) +
3 − 27)]
11
1050𝑁2 (𝐽1
519
673750𝑁4 (𝐽1
5 − 243)] + 𝑊𝐻(𝐽) 
where  the  hydrostatic  work  term  is  in  terms  of  the  bulk  modulus,  K,  and  the  third 
invariant, J, as: 
Rate  effects  are  taken  into  account  through  linear  viscoelasticity  by  a  convolution 
integral of the form: 
𝑊𝐻(𝐽) =
(𝐽 − 1)2 
𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)
∂𝜀𝑘𝑙
∂𝜏
𝑑𝜏 
or in terms of the second Piola-Kirchhoff stress, 𝑆𝑖𝑗, and Green's strain tensor, 𝐸𝑖𝑗,
𝑆𝑖𝑗 = ∫ 𝐺𝑖𝑗𝑘𝑙
(𝑡 − 𝜏)
∂𝐸𝑘𝑙
∂𝜏
𝑑𝜏 
where  𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)  and  𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏)  are  the  relaxation  functions  for  the  different  stress 
measures.    This  stress  is  added  to  the  stress  tensor  determined  from  the  strain  energy 
functional. 
If we wish to include only simple rate effects, the relaxation function is represented by 
six terms from the Prony series: 
given by, 
𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚𝑒−𝛽𝑡
𝑚=1
𝑔(𝑡) = ∑ 𝐺𝑖𝑒−𝛽𝑖𝑡
𝑖=1
This  model  is  effectively  a  Maxwell  fluid  which  consists  of  a  dampers  and  springs  in 
series.  We  characterize this in the input by  shear moduli, 𝐺𝑖, and  decay constants,  𝛽𝑖.  
The viscoelastic behavior is optional and an arbitrary number of terms may be used.
*MAT_128 
This is Material Type 128.  This material model provides a heart tissue model described 
in the paper by Walker et al [2005] as interpreted by Kay Sun.  It is backward compatible 
with an earlier heart tissue model described in the paper by Guccione, McCulloch, and 
Waldman [1991].  Both models are transversely isotropic. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
C 
F 
4 
B1 
F 
5 
B2 
F 
6 
B3 
F 
7 
P 
F 
8 
B 
F 
Skip to Card 3 to activate older Guccione, McCulloch, and Waldman [1991] model. 
  Card 2 
Variable 
1 
L0 
2 
3 
CA0MAX 
LR 
4 
M 
5 
BB 
6 
7 
8 
CA0 
TMAX 
TACT 
Type 
F 
  Card 3 
1 
I 
2 
Variable 
AOPT 
MACF 
Type 
F 
I 
3 
4 
5 
6 
7 
8 
  Card 4 
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
3 
ZP 
F 
4 
A1 
F 
5 
A2 
F 
6 
A3 
F 
7
Variable 
1 
V1 
Type 
F 
  VARIABLE   
MID 
*MAT_HEART_TISSUE 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
7 
8 
BETA 
F 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density 
C 
B1 
B2 
B3 
P 
B 
L0 
Diastolic material coefficient. 
𝑏1, diastolic material coefficient. 
𝑏2, diastolic material coefficient. 
𝑏3, diastolic material coefficient. 
Pressure in the muscle tissue 
Systolic material coefficient.  Omit for the earlier model. 
𝑙0,  sacromere  length  at  which  no  active  tension  develops.    Omit
for the earlier model. 
CA0MAX 
(𝐶𝑎0)max, maximum peak intracellular calcium concentrate.  Omit
for the earlier model.
LR 
M 
BB 
CA0 
TMAX 
TACT 
𝑙𝑅, Stress-free sacromere length.  Omit for the earlier model.
Systolic material coefficient.  Omit for the earlier model.
Systolic material coefficient.  Omit for the earlier model. 
𝐶𝑎0, peak intracellular calcium concentration.  Omit for the earlier
model. 
𝑇max,  maximum  isometric  tension  achieved  at  the  longest
sacromere length.  Omit for the earlier model.
𝑡act, time at which active contraction initiates.  Omit for the earlier
model
VARIABLE   
AOPT 
DESCRIPTION
Material axes option : 
EQ.0.0:  locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES. 
EQ.1.0:  locally orthotropic with material axes determined by a
point  in  space  and  the  global  location  of  the  element
center; this is the a-direction. 
EQ.2.0:  globally orthotropic with material axes determined by 
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0:  locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the 
element normal. 
EQ.4.0:  locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector  v,  and
an originating point, P, which define the centerline ax-
is. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
MACF 
Material axes change flag for brick elements: 
EQ.1:  No change, default, 
EQ.2:  switch material axes a and b, 
EQ.3:  switch material axes a and c, 
EQ.4:  switch material axes b and c. 
XP, YP, ZP 
xp yp zp, define coordinates of point p for AOPT = 1 and 4. 
A1, A2, A3 
a1 a2 a3, define components of vector a for AOPT = 2. 
D1, D2, D3 
d1 d2 d3, define components of vector d for AOPT = 2. 
V1, V2, V3 
v1 v2 v3, define components of vector v for AOPT = 3 and 4.
Material  angle  in  degrees  for  AOPT = 3,  may  be  overridden  on 
the element card, see *ELEMENT_SOLID_ORTHO. 
*MAT_128 
  VARIABLE   
BETA 
Remarks: 
1.  The  tissue  model  is  described  in  terms  of  the  energy  functional  that  is 
transversely isotropic with respect to the local fiber direction, 
(𝑒𝑄 − 1) 
𝑊 =
𝑄 = 𝑏𝑓 𝐸11
2 + 𝑏𝑡(𝐸22
2 + 𝐸33
2 + 𝐸23
2 + 𝐸32
2 ) + 𝑏𝑓𝑠(𝐸12
2 + 𝐸21
2 + 𝐸13
2 + 𝐸31
2 ) 
with 𝐶, 𝑏𝑓 , 𝑏𝑡, and 𝑏𝑓𝑠 material parameters and E the Lagrange-Green strains. 
The systolic  contraction was modeled as the sum of the passive stress derived 
from  the  strain  energy  function  and  an  active  fiber  directional  component,  𝑇0, 
which is a function of time, t, 
− 𝑝𝐽𝐶−1 + 𝑇0{𝑡, 𝐶𝑎0, 𝑙}
𝑆 =
𝜎 =
∂𝑊
∂𝐸
𝐹𝑆𝐹𝑇
with  𝑆  the  second  Piola-Kirchoff  stress  tensor,    𝐶  the  right  Cauchy-Green  de-
formation tensor, J the Jacobian of the deformation gradient tensor 𝐹, and 𝜎 the 
Cauchy stress tensor. 
The active fiber directional stress component is defined by a time-varying elas-
tance model, which at end-systole, is reduced to 
𝑇0 = 𝑇max
𝐶𝑎0
2 + 𝐸𝐶𝑎50
2 𝐶𝑡 
𝐶𝑎0
with  𝑇max  the  maximum  isometric  tension  achieved  at  the  longest  sacromere 
length  and  maximum  peak  intracellular  calcium  concentration.    The  length-
dependent calcium sensitivity and internal variable is given by, 
𝐸𝐶𝑎50 =
(𝐶𝑎0)max
√exp[𝐵(𝑙 − 𝑙0] − 1
𝐶𝑡 = 1/2(1 − cos 𝑤) 
𝑙 = 𝑙𝑅√2𝐸11 + 1
𝑤 = 𝜋
0.25 + 𝑡𝑟
𝑡𝑟
𝑡𝑟 = 𝑚𝑙 + 𝑏𝑏 
A  cross-fiber,  in-plane  stress  equivalent  to  40%  of  that  along  the  myocardial 
fiber direction is added. 
2.  The earlier tissue model is described in terms of the energy functional in terms 
of the Green strain components, 𝐸𝑖𝑗, 
𝑊(𝐸) =
(𝑒𝑄 − 1) +
𝑄 = 𝑏1𝐸11
2 + 𝐸33
2 + 𝑏2(𝐸22
𝑃(𝐼3 − 1) 
2 + 𝐸23
2 + 𝐸32
2 ) + 𝑏3(𝐸12
2 + 𝐸21
2 + 𝐸13
2 + 𝐸31
2 ) 
The  Green  components  are  modified  to  eliminate  any  effects  of  volumetric 
work  following  the  procedures  of  Ogden.    See  the  paper  by  Guccione  et  al 
[1991] for more detail.
*MAT_LUNG_TISSUE 
This is Material Type 129.  This material model provides a hyperelastic model for heart 
tissue, see [Vawter 1980] combined optionally with linear viscoelasticity as outlined by 
[Christensen 1980]. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
  Card 2 
Variable 
1 
C1 
Type 
F 
2 
C2 
F 
3 
K 
F 
3 
4 
C 
F 
4 
5 
6 
7 
8 
DELTA 
ALPHA 
BETA 
F 
5 
F 
6 
F 
7 
8 
LCID 
TRAMP 
NT 
F 
F 
F 
Viscoelastic Constant Cards.  Up to 6 cards may be input.  A keyword card (with a 
“*” in column 1) terminates this input if less than 6 cards are used. 
  Card 3 
Variable 
Type 
1 
GI 
F 
2 
3 
4 
5 
6 
7 
8 
BETAI 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
K 
C 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Bulk modulus 
Material coefficient. 
DELTA 
Δ, material coefficient. 
ALPHA 
𝛼, material coefficient.
VARIABLE   
DESCRIPTION
BETA 
𝛽, material coefficient. 
C1 
C2 
Material coefficient. 
Material coefficient. 
LCID 
Optional load curve ID of relaxation curve 
If  constants  𝐺𝑖  and  𝛽𝑖  are  determined  via  a  least  squares  fit. 
This  relaxation  curve  is  shown  in  Figure  M76-1.    This  model 
ignores the constant stress. 
TRAMP 
Optional ramp time for loading. 
NT 
Number of Prony series terms in optional fit.  If zero, the default
is  6.    Currently,  the  maximum  number  is  6.    Values  less  than  6, 
possibly  3 - 5  are  recommended,  since  each  term  used  adds
significantly  to  the  cost.    Caution  should  be  exercised  when
taking the results from the fit.  Always check the results of the fit
in the output file.  Preferably, all generated coefficients should be 
positive.    Negative  values  may  lead  to  unstable  results.    Once  a
satisfactory  fit  has  been  achieved  it  is  recommended  that  the
coefficients  which  are  written  into  the  output  file  be  input  in
future runs. 
Gi 
Optional shear relaxation modulus for the ith term 
BETAi 
Optional decay constant if ith term 
Remarks: 
The  material  is  described  by  a  strain  energy  functional  expressed  in  terms  of  the 
invariants of the Green Strain: 
𝑊(𝐼1, 𝐼2) =
2Δ
𝑒(𝛼𝐼1
2+𝛽𝐼2) +
12𝐶1
Δ(1 + 𝐶2)
[𝐴(1+𝐶2) − 1] 
𝐴2 =
(𝐼1 + 𝐼2) − 1 
where  the  hydrostatic  work  term  is  in  terms  of  the  bulk  modulus,  K,  and  the  third 
invariant, J, as: 
𝑊𝐻(𝐽) =
(𝐽 − 1)2
Rate  effects  are  taken  into  account  through  linear  viscoelasticity  by  a  convolution 
integral of the form: 
𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙
(𝑡 − 𝜏)
∂𝜀𝑘𝑙
∂𝜏
𝑑𝜏 
or in terms of the second Piola-Kirchhoff stress, 𝑆𝑖𝑗, and Green's strain tensor, 𝐸𝑖𝑗, 
𝑆𝑖𝑗 = ∫ 𝐺𝑖𝑗𝑘𝑙
(𝑡 − 𝜏)
∂ 𝐸𝑘𝑙
∂𝜏
𝑑𝜏 
where  𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)  and  𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏)    are  the  relaxation  functions  for  the  different  stress 
measures.    This  stress  is  added  to  the  stress  tensor  determined  from  the  strain  energy 
functional. 
If we wish to include only simple rate effects, the relaxation function is represented by 
six terms from the Prony series: 
given by, 
𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚
𝑚=1
𝑒−𝛽 𝑡 
𝑔(𝑡) = ∑ 𝐺𝑖𝑒−𝛽𝑖 𝑡
𝑖=1
This  model  is  effectively  a  Maxwell  fluid  which  consists  of  a  dampers  and  springs  in 
series.  We  characterize this in the input by  shear moduli, 𝐺𝑖, and  decay constants,  𝛽𝑖.  
The viscoelastic behavior is optional and an arbitrary number of terms may be used.
*MAT_130 
This  is  Material  Type  130.    This  model  is  available  the  Belytschko-Tsay  and  the  C0 
triangular  shell  elements  and  is  based  on  a  resultant  stress  formulation.    In-plane 
behavior is treated separately from bending in order to model perforated materials such 
as  television  shadow  masks.    If  other  shell  formulations  are  specified,  the  formulation 
will  be  automatically  switched  to  Belytschko-Tsay.    As  implemented,  this  material 
model cannot be used with user defined integration rules. 
NOTE: This material does not support specification of a ma-
terial  angle,  𝛽𝑖,  for  each  through-thickness  integra-
tion point of a shell. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
YS 
F 
3 
4 
EP 
F 
4 
5 
6 
7 
8 
5 
6 
7 
8 
Variable 
E11P 
E22P 
V12P 
V21P 
G12P 
G23P 
G31P 
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
8 
Variable 
E11B 
E22B 
V12B 
V21B 
G12B 
AOPT 
Type 
F 
  Card 4 
1 
F 
2 
F 
3 
Variable 
Type 
F 
F 
F 
4 
A1 
F 
5 
A2 
F 
6 
A3 
F 
7
Variable 
1 
V1 
Type 
F 
*MAT_SPECIAL_ORTHOTROPIC 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
7 
8 
BETA 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
YS 
EP 
E11P 
E22P 
V12P 
V11P 
G12P 
G23P 
G31P 
E11B 
E22B 
V12B 
V21B 
G12B 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Yield  stress.    This  parameter  is  optional  and  is  approximates the
yield condition.  Set to zero if the behavior is elastic.   
Plastic hardening modulus. 
𝐸11𝑝, for in plane behavior. 
𝐸22𝑝, for in plane behavior. 
𝜈12𝑝, for in plane behavior. 
𝜈11𝑝, for in plane behavior. 
𝐺12𝑝, for in plane behavior. 
𝐺23𝑝, for in plane behavior. 
𝐺31𝑝, for in plane behavior. 
𝐸11𝑝, for bending behavior. 
𝐸22𝑝, for bending behavior. 
𝜈12𝑏, for bending behavior. 
𝜈21𝑏, for bending behavior. 
𝐺12𝑏, for bending behavior.
VARIABLE   
AOPT 
DESCRIPTION
Material  axes  option  : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES,  and  then  rotated  about  the  shell  ele-
ment normal by an angle BETA. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  𝐯  with  the 
element normal. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID 
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
A1, A2, A3 
(𝑎1, 𝑎2, 𝑎3), define components of vector 𝐚 for AOPT = 2. 
D1, D2, D3 
(𝑑1, 𝑑2, 𝑑3), define components of vector 𝐝 for AOPT = 2. 
V1 ,V2, V3 
(𝑣1, 𝑣2, 𝑣3), define components of vector 𝐯 for AOPT = 3. 
BETA 
Material angle in degrees for AOPT = 0 and 3, may be overridden 
on the element card, see *ELEMENT_SHELL_BETA. 
Remarks: 
The in-plane elastic matrix for in-plane, plane stress behavior is given by: 
𝐂in plane =
𝑄11𝑝        𝑄12𝑝      0        0        0
⎤
𝑄12𝑝        𝑄22𝑝      0        0        0
⎥
⎥
    0          0        𝑄44𝑝      0        0
⎥
⎥
    0          0        0        𝑄55𝑝      0
⎥
    0          0        0        0        𝑄66𝑝⎦
⎡
⎢
⎢
⎢
⎢
⎢
⎣
The terms 𝑄𝑖𝑗𝑝 are defined as:
𝑄11𝑝 =
𝑄22𝑝 =
𝑄12𝑝 =
𝐸11𝑝
1 − 𝜈12𝑝𝜈21𝑝
𝐸22𝑝
1 − 𝜈12𝑝𝜈21𝑝
𝜈12𝑝𝐸11𝑝
1 − 𝜈12𝑝𝜈21𝑝
𝑄44𝑝 = 𝐺12𝑝 
𝑄55𝑝 = 𝐺23𝑝 
𝑄66𝑝 = 𝐺31𝑝 
The elastic matrix for bending behavior is given by: 
𝐂bending =
𝑄11𝑏        𝑄12𝑏      0
⎤
⎡
𝑄12𝑏        𝑄22𝑏      0
⎥
⎢
    0          0        𝑄44𝑏⎦
⎣
The terms 𝑄𝑖𝑗𝑝 are similarly defined. 
Because this is a resultant formulation, nothing is written to the six stress slots of d3plot.  
Resultant forces and moments may be written to elout and to dynain in place of the six 
stresses.      The  first  two  extra  history  variables  may  be  used  to  complete  output  of  the 
eight resultants to elout and dynain.
*MAT_ISOTROPIC_SMEARED_CRACK 
This is Material Type 131.  This model was developed by Lemmen and Meijer [2001] as 
a smeared crack model for isotropic materials.  This model is available of solid elements 
only  and  is  restricted  to  cracks  in  the  x-y  plane.    Users  should  choose  other  models 
unless they have the report by Lemmen and Meijer [2001]. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
6 
ISPL 
SIGF 
I 
F 
7 
GK 
F 
8 
SR 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s modulus 
Poisson’s ratio 
ISPL 
Failure option: 
EQ.0: Maximum principal stress criterion 
EQ.5: Smeared crack model 
EQ.6: Damage model based on modified von Mises strain 
SIGF 
Peak stress. 
GK 
SR 
Critical energy release rate. 
Strength ratio. 
Remarks: 
The  following  documentation  is  taken  nearly  verbatim  from  the  documentation  of 
Lemmen and Meijer [2001]. 
Three methods are offered to model progressive failure.  The maximum principal stress 
criterion  detects  failure  if  the  maximum  (most  tensile)  principal  stress  exceeds  𝜎max.  
Upon failure, the material can no longer carry stress.
The second failure model is the smeared crack model with linear softening stress-strain 
using  equivalent  uniaxial  strains.    Failure  is  assumed  to  be  perpendicular  to  the 
principal  strain  directions.    A  rotational crack  concept  is  employed  in  which  the  crack 
directions  are  related  to  the  current  directions  of  principal  strain.    Therefore  crack 
directions may rotate in time.  Principal stresses are expressed as 
E̅̅̅̅̅1
⎡
⎢⎢
⎣
E̅̅̅̅̅1𝜀̃1
⎟⎟⎟⎞
E̅̅̅̅̅2𝜀̃2
E̅̅̅̅̅3𝜀̃3⎠
⎤
⎥⎥
E̅̅̅̅̅3⎦
𝜎1
𝜎2
𝜎3⎠
𝜀̃1
𝜀̃2
𝜀̃3⎠
E̅̅̅̅̅2
(131.1)
⎟⎟⎞ =
⎟⎞ =
⎜⎜⎜⎛
⎝
⎜⎜⎛
⎝
⎜⎛
⎝
with E̅̅̅̅̅1, E̅̅̅̅̅2 and E̅̅̅̅̅3 secant stiffness in the terms that depend on internal variables. 
In  the  model  developed  for  DYCOSS  it  has  been  assumed  that  there  is  no  interaction 
between the three directions in which case stresses simply follow from 
𝜎𝑗(𝜀̃𝑗) =
⎧E𝜀̃𝑗
{{{
⎨
{{{
⎩
𝜎̅̅̅̅̅ (1 −
𝑖𝑓
0 ≤ 𝜀̃𝑗 ≤ 𝜀̃𝑗,ini
𝜀̃𝑗 − 𝜀̃𝑗,ini
𝜀̃𝑗,ult − 𝜀̃𝑗,ini
) 𝑖𝑓
𝜀̃𝑗,ini < 𝜀̃𝑗 ≤ 𝜀̃𝑗,ult
(131.2)
𝑖𝑓
𝜀̃𝑗 > 𝜀̃𝑗,ult
with  𝜎̅̅̅̅̅  the  ultimate  stress,  𝜀̃𝑗,inithe  damage  threshold,  and  𝜀̃𝑗,ultthe  ultimate  strain  in  j-
direction.  The damage threshold is defined as 
𝜀̃𝑗,ini =
𝜎̅̅̅̅̅
(131.3)
The ultimate strain is obtained by relating the crack growth energy and the dissipated 
energy 
∫ ∫ 𝜎̅̅̅̅̅𝑑𝜀̃𝑗,ult𝑑𝑉 = 𝐺𝐴
(131.4)
with G the energy release rate, V the element volume and A the area perpendicular to 
the  principal  strain  direction.    The  one  point  elements  LS-DYNA  have  a  single 
integration point and the integral over the volume may be replaced by the volume.  For 
linear softening it follows 
𝜀̃𝑗,ult =
2𝐺𝐴
𝑉𝜎̅̅̅̅̅
(131.5)
The  above  formulation  may  be  regarded  as  a  damage  equivalent  to  the  maximum 
principle stress criterion. 
The third model is a damage model represented by Brekelmans et.  al [1991].  Here the 
Cauchy stress tensor 𝜎 is expressed as 
𝜎 = (1 − 𝐷)E𝜀
(131.6)
where  D  represents  the  current  damage  and  the  factor  (1-D)  is  the  reduction  factor 
caused by damage.  The scalar damage variable is expressed as function of a so-called 
damage equivalent strain 𝜀𝑑
𝐷 = 𝐷(𝜀𝑑) = 1 −
𝜀ini(𝜀ult − 𝜀𝑑)
𝜀𝑑(𝜀ult − 𝜀ini)
and 
𝜀𝑑 =
𝑘 − 1
2𝑘(1 − 2𝑣)
𝐽1 +
2𝑘
√(
𝑘 − 1
1 − 2𝑣
𝐽1)
+
6𝑘
(1 + 𝑣)2 𝐽2
(131.7)
(131.8)
where the constant k represents the ratio of the strength in tension over the strength in 
compression 
𝑘 =
𝜎ult ,tension
𝜎ult, compression
(131.9)
J1  resp.  J2  are  the  first  and  second  invariant  of  the  strain  tensor  representing  the 
volumetric and the deviatoric straining respectively 
𝐽1 = tr(𝜀)
𝐽2 = tr(𝜀 ⋅ 𝜀) −
[𝑡𝑟(𝜀)]2
(131.10)
If  the  compression  and  tension  strength  are  equal  the  dependency  on  the  volumetric 
strain  vanishes  in  (8)  and  failure  is  shear  dominated.    If  the  compressive  strength  is 
much  larger  than  the  strength  in  tension,  k  becomes  small  and  the  J1  terms  in  (131.8) 
dominate the behavior.
*MAT_ORTHOTROPIC_SMEARED_CRACK 
This  is  Material  Type  132.    This  material  is  a  smeared  crack  model  for  orthotropic 
materials. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
EA 
F 
3 
4 
EB 
F 
4 
5 
EC 
F 
5 
6 
7 
8 
PRBA 
PRCA 
PRCB 
F 
6 
F 
7 
F 
8 
Variable 
UINS 
UISS 
CERRMI  CERRMII 
IND 
ISD 
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
F 
4 
Variable 
GAB 
GBC 
GCA 
AOPT 
Type 
F 
F 
F 
F 
  Card 4 
Variable 
1 
XP 
Type 
F 
  Card 5 
Variable 
1 
V1 
Type 
F 
2 
YP 
F 
2 
V2 
F 
3 
ZP 
F 
3 
V3 
F 
4 
A1 
F 
4 
D1 
F 
I 
5 
5 
A2 
F 
5 
D2 
F 
I 
6 
6 
A3 
F 
6 
D3 
F 
7 
8 
7 
8 
MACF 
I 
7 
8 
BETA 
REF 
F
VARIABLE   
DESCRIPTION
MID 
RO 
EA 
EB 
EC 
PRBA 
PRCA 
PRCB 
UINS 
UISS 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Ea, Young’s modulus in a-direction. 
Eb, Young’s modulus in b-direction. 
Ec, Young’s modulus in c-direction 
ba, Poisson’s ratio ba. 
νca, Poisson’s ratio ca. 
cb, Poisson’s ratio cb. 
Ultimate  interlaminar normal stress. 
Ultimate interlaminar shear stress. 
CERRMI 
Critical energy release rate mode I 
CERRMII 
Critical energy release rate mode II 
IND 
Interlaminar normal direction : 
EQ.1.0: Along local a axis 
EQ.2.0: Along local b axis 
EQ.3.0: Along local c axis 
ISD 
Interlaminar shear direction : 
EQ.4.0: Along local ab axis 
EQ.5.0: Along local bc axis 
EQ.6.0: Along local ca axis 
GAB 
GBC 
GCA 
Gab, shear modulus ab. 
Gbc, shear modulus bc. 
Gca, shear modulus ca.
*MAT_ORTHOTROPIC_SMEARED_CRACK 
DESCRIPTION
AOPT 
Material axes option, see Figure 2.1. 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes as shown in Figure 2.1.  Nodes 1, 2, and
4 of an element are identical to the nodes used for the
definition  of  a  coordinate  system  as  by  *DEFINE_CO-
ORDINATE_NODES. 
EQ.1.0: locally orthotropic with material axes determined by a 
point  in  space  and  the  global  location  of  the  element
center;  this  is  the  a-direction.    This  option  is  for  solid 
elements only. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the 
element  normal.    The  plane  of  a  solid  element  is  the
midsurface between the inner surface and outer surface
defined by the first four nodes and the last four nodes
of the connectivity of the element, respectively. 
EQ.4.0: locally  orthotropic  in  cylindrical  coordinate  system 
with  the  material  axes  determined  by  a  vector  v,  and
an originating point, P, which define the centerline ax-
is.  This option is for solid elements only. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
XP YP ZP 
Define coordinates of point p for AOPT = 1 and 4. 
A1 A2 A3 
Define components of vector a for AOPT = 2.
VARIABLE   
DESCRIPTION
MACF 
Material axes change flag for brick elements: 
EQ.1: No change, default, 
EQ.2: switch material axes a and b, 
EQ.3: switch material axes a and c, 
EQ.4: switch material axes b and c. 
V1 V2 V3 
Define components of vector v for AOPT = 3 and 4. 
D1 D2 D3 
Define components of vector d for AOPT = 2: 
BETA 
REF 
Material  angle  in  degrees  for  AOPT = 3,  may  be  overridden  on 
the element card, see *ELEMENT_SOLID_ORTHO. 
Use  reference  geometry  to  initialize  the  stress  tensor.    The
reference  geometry  is  defined  by  the  keyword:  *INITIAL_-
FOAM_REFERENCE_GEOMETRY . 
EQ.0.0: off, 
EQ.1.0: on. 
Remarks: 
This is an orthotropic material with optional delamination failure for brittle composites.  
The  elastic  formulation  is  identical  to  the  DYNA3D  model  that  uses  total  strain 
formulation.  The constitutive matrix C that relates to global components of stress to the 
global components of strain is defined as: 
C = T𝑇C𝐿T 
where T is the transformation matrix between the local material coordinate system and 
the  global  system  and  C𝐿is  the  constitutive  matrix  defined  in  terms  of  the  material 
constants of the local orthogonal material axes a, b, and c . 
Failure  is  described  using  linear  softening  stress  strain  curves  for  interlaminar  normal 
and interlaminar shear direction.  The current implementation for failure is essentially 
2-D.    Damage  can  occur  in  interlaminar  normal  direction  and  a  single  interlaminar 
shear  direction.    The  orientation  of  these  directions  w.r.t.    the  principal  material 
directions have to be specified by the user. 
Based  on  specified  values  for  the  ultimate  stress  and  the  critical  energy  release  rate 
bounding surfaces are defined 
𝑓𝑛 = 𝜎𝑛 − 𝜎̅̅̅̅̅𝑛(𝜀𝑛)
𝑓𝑠 = 𝜎𝑠 − 𝜎̅̅̅̅̅𝑠(𝜀𝑠) 
where  the  subscripts  n  and  s  refer  to  the  normal  and  shear  component.    If  stresses 
exceed the bounding surfaces inelastic straining occurs.  The ultimate strain is obtained 
by relating the crack growth energy and the dissipated energy.  For solid elements with 
a single integration point it can be derived 
𝜀𝑖,ult =
2𝐺𝑖𝐴
𝑉𝜎𝑖,ult
with 𝐺𝑖the critical energy release rate, 𝑉the element volume, A the area perpendicular 
to the active normal direction and 𝜎𝑖, ult the ultimate stress.  For the normal component 
failure  can  only  occur  under  tensile  loading.    For  shear  component  the  behavior  is 
symmetric  around  zero.    The  resulting  stress  bounds  are  depicted  in  Figure  M132-1.  
Unloading is modeled with a Secant stiffness. 
n,ult
ult
Figure  M132-1.    Shows  stress  bounds  for  the  active  normal  component  (left)
and the archive shear component (right). 
-τ
ult
*MAT_133 
This  is  Material  Type  133.    This  model  was  developed  by  Barlat  et  al.    [2003]  to 
overcome  some  shortcomings  of  the  six  parameter  Barlat  model  implemented  as 
material  33  (MAT_BARLAT_YLD96)  in  LS-DYNA.    This  model  is  available  for  shell 
elements only. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
  Card 2 
Variable 
Type 
1 
K 
F 
2 
E0 
F 
3 
E 
F 
3 
N 
F 
4 
PR 
F 
4 
C 
F 
5 
FIT 
F 
5 
P 
F 
6 
7 
8 
BETA 
ITER 
ISCALE 
F 
8 
F 
6 
HARD 
F 
F 
7 
A 
F 
Chaboche-Roussilier Card.  Additional Card for A < 0. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CRC1 
CRA1 
CRC2 
CRA2 
CRC3 
CRA3 
CRC4 
CRA4 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Direct Material Parameter Card.  Additional card for FIT = 0. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ALPHA1 
ALPHA2 
ALPHA3 
ALPHA4 
ALPHA5 
ALPHA6 
ALPHA7 
ALPHA8 
Type 
F 
F 
F 
F 
F 
F 
F
Test Data Card 1.  Additional Card for FIT = 1. 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SIG00 
SIG45 
SIG90 
R00 
R45 
R90 
Type 
F 
F 
F 
F 
F 
F 
Test Data Card 2.  Additional Card for FIT = 1. 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SIGXX 
SIGYY 
SIGXY 
DXX 
DYY 
DXY 
Type 
F 
F 
F 
F 
F 
F 
Hansel Hardening Card 1.  Additional Card for HARD = 3. 
  Card 7 
Variable 
1 
CP 
Type 
F 
2 
T0 
F 
3 
4 
5 
6 
7 
8 
TREF 
TA0 
F 
F 
Hansel Hardening Card 2.  Additional Card for HARD = 3. 
  Card 8 
Variable 
Type 
1 
A 
F 
2 
B 
F 
3 
C 
F 
4 
D 
F 
5 
P 
F 
6 
Q 
F 
7 
8 
E0MART 
VM0 
F 
F 
Hansel Hardening Card 3.  Additional Card for HARD = 3. 
  Card 9 
1 
2 
Variable 
AHS 
BHS 
Type 
F 
F 
3 
M 
F 
4 
N 
F 
5 
6 
EPS0 
HMART 
F 
F 
7 
K1 
F 
8 
K2
Card 10 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
AOPT 
OFFANG 
P4 
HTFLAG 
HTA 
HTB 
HTC 
HTD 
Type 
F 
  Card 11 
1 
Variable 
Type 
  Card 12 
Variable 
1 
V1 
Type 
F 
  VARIABLE   
MID 
RO 
E 
PR 
FIT 
F 
F 
F 
F 
2 
2 
V2 
F 
F 
3 
3 
V3 
F 
4 
A1 
F 
4 
D1 
F 
5 
A2 
F 
5 
D2 
F 
DESCRIPTION
F 
7 
F 
8 
7 
8 
6 
A3 
F 
6 
D3 
USRFAIL 
F 
F 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s modulus 
LE.0:  -E is load curve ID for Young’s modulus vs.  plastic strain
Poisson’s ratio 
Material parameter fit flag: 
EQ.0.0: Material parameters are used directly on card 3. 
EQ.1.0: Material  parameters  are  determined  from  test  data  on
cards 3 and 4 
BETA 
Hardening  parameter.    Any  value  ranging  from  0  (isotropic
hardening) to 1 (kinematic hardening) may be input.
*MAT_BARLAT_YLD2000 
DESCRIPTION
ITER 
Plastic iteration flag: 
EQ.0.0: Plane stress algorithm for stress return 
EQ.1.0: Secant iteration algorithm for stress return 
ITER  provides  an  option  of  using  three  secant  iterations  for
determining  the  thickness  strain  increment  as  experiments  have
shown  that  this  leads  to  a  more  accurate  prediction  of  shell
thickness  changes  for  rapid  processes.    A  significant  increase  in
computation time is incurred with this option so it should be used
only for applications associated with high rates of loading and/or
for implicit analysis. 
ISCALE 
Yield locus scaling flag: 
EQ.0.0: Scaling  on  –  reference  direction = rolling  direction 
(default) 
EQ.1.0: Scaling off – reference direction arbitrary 
K 
Material parameter: 
HARD.EQ.1.0:  𝑘, strength coefficient for exponential hardening
HARD.EQ.2.0:  𝑎 in Voce hardening law 
HARD.EQ.4.0:  𝑘, strength coefficient for Gosh hardening 
HARD.EQ.5.0:  𝑎 in Hocket-Sherby hardening law 
E0 
Material parameter: 
HARD.EQ.1.0:  𝑒0, strain at yield for exponential hardening 
HARD.EQ.2.0:  𝑏 in Voce hardening law 
HARD.EQ.4.0:  𝜀0, strain at yield for Gosh hardening 
HARD.EQ.5.0:  𝑏 in Hocket-Sherby hardening law 
N 
Material parameter: 
HARD.EQ.1.0:  𝑛, exponent for exponential hardening 
HARD.EQ.2.0:  𝑐 in Voce hardening law 
HARD.EQ.4.0:  𝑛, exponent for Gosh hardening 
HARD.EQ.5.0:  𝑐 in Hocket-Sherby hardening law 
C 
Cowper-Symonds strain rate parameter, C, see formula below.
VARIABLE   
DESCRIPTION
P 
Cowper-Symonds strain rate parameter, 𝑝. 
𝜎𝑦
𝑣(𝜀𝑝, 𝜀̇𝑝) = 𝜎𝑦(𝜀𝑝)
⎜⎛1 + [
⎝
𝜀̇𝑝
1/𝑝
]
⎟⎞ 
⎠
HARD 
Hardening law: 
EQ.1.0: Exponential hardening: 𝜎𝑦 = 𝑘(𝜀0 + 𝜀𝑝)
EQ.2.0: Voce hardening: 𝜎𝑦 = 𝑎 − 𝑏𝑒−𝑐𝜀𝑝
EQ.3.0: Hansel hardening 
EQ.4.0: Gosh hardening: 𝜎𝑦 = 𝑘(𝜀0 + 𝜀𝑝)
− 𝑝 
EQ.5.0: Hocket-Sherby hardening: 𝜎𝑦 = 𝑎 − 𝑏𝑒−𝑐𝜀𝑝
LT.0.0:  Absolute  value  defines  load  curve  ID  or  table  ID  with 
yield stress as functions of plastic strain and in the lat-
ter case also plastic strain rate. 
A 
CRCn 
CRAn 
Flow potential exponent.  For face centered cubic (FCC) materials
A = 8  is  recommended  and  for  body  centered  cubic  (BCC)
materials A = 6 may be used. 
Chaboche-Rousselier  kinematic  hardening  parameters,  see
remarks. 
Chaboche-Rousselier  kinematic  hardening  parameters,  see
remarks. 
ALPHA1 
𝛼1, see equations below 
⋮ 
⋮ 
ALPHA8 
𝛼8, see equations below 
SIG00 
SIG45 
SIG90 
R00 
R45 
Yield stress in 00 direction 
Yield stress in 45 direction 
Yield stress in 90 direction 
𝑅-value in 00 direction 
𝑅-value in 45 direction
*MAT_BARLAT_YLD2000 
DESCRIPTION
R90 
𝑅-value in 90 direction 
SIGXX 
SIGYY 
SIGXY 
DXX 
DYY 
DXY 
CP 
T0 
TREF 
TA0 
A 
B 
C 
D 
P 
Q 
𝑥𝑥-component of stress on yield surface . 
𝑦𝑦-component of stress on yield surface . 
𝑥𝑦-component of stress on yield surface . 
𝑥𝑥-component of tangent to yield surface . 
𝑦𝑦-component of tangent to yield surface . 
𝑥𝑦-component of tangent to yield surface . 
Adiabatic temperature calculation option: 
EQ.0.0: Adiabatic temperature calculation is disabled. 
GT.0.0:  CP  is  the  specific  heat  𝐶𝑝.    Adiabatic  temperature 
calculation is enabled. 
Initial  temperature  𝑇0  of  the  material  if  adiabatic  temperature 
calculation is enabled. 
Reference  temperature  for  output  of  the  yield  stress  as  history
variable. 
Reference  temperature  𝑇𝐴0,  the  absolute  zero  for  the  used 
temperature scale, e.g.  -273.15 if the Celsius scale is used and 0.0 
if the Kelvin scale is used. 
Martensite rate equation parameter 𝐴, see equations below. 
Martensite rate equation parameter 𝐵, see equations below. 
Martensite rate equation parameter 𝐶, see equations below. 
Martensite rate equation parameter 𝐷, see equations below. 
Martensite rate equation parameter 𝑝, see equations below. 
Martensite rate equation parameter 𝑄, see equations below. 
E0MART 
Martensite rate equation parameter 𝐸0(mart) , see equations below.
VARIABLE   
VM0 
DESCRIPTION
The  initial  volume  fraction  of  martensite  0.0 < 𝑉𝑚0 < 1.0  may  be 
initialised using two different methods: 
GT.0.0: 𝑉𝑚0 is set to VM0. 
LT.0.0:  Can  be  used  only  when  there  are  initial  plastic  strains
εp  present,  e.g. 
  when  using  *INITIAL_STRESS_-
SHELL.    The  absolute  value  of  VM0  is  then  the  load
curve  ID  for  a  function  f  that  sets  𝑉𝑚0 = 𝑓 (𝜀𝑝).  The 
function  f  must  be  a  monotonically  nondecreasing
function of 𝜀𝑝.  
AHS 
BHS 
M 
N 
Hardening law parameter𝐴HS, see equations below. 
Hardening law parameter𝐵HS, see equations below. 
Hardening law parameter 𝑚, see equations below. 
Hardening law parameter 𝑛, see equations below. 
EPS0 
Hardening law parameter 𝜀0, see equations below. 
HMART 
Hardening law parameter Δ𝐻𝛾→𝛼’, see equations below. 
K1 
K2 
Hardening law parameter 𝐾1, see equations below. 
Hardening law parameter 𝐾2, see equations below 
AOPT 
Material axes option: 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes as shown in Figure M133-1.  Nodes 1, 2, 
and 4 of an element are identical to the  nodes used for
the definition of a coordinate system as by *DEFINE_-
COORDINATE_NODES 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR 
EQ.3.0: locally  orthotropic  material  axes  determined  by
offsetting  the  material  axes  by  an  angle,  OFFANG,
from  a  line  determined  by  taking  the  cross  product  of
the  vector  v  with  the  normal  to  the  plane  of  the  ele-
ment. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES,
*MAT_BARLAT_YLD2000 
DESCRIPTION
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
OFFANG 
Offset angle for AOPT = 3 
P4 
Material parameter: 
HARD.EQ.4.0:  𝑝 in Gosh hardening law 
HARD.EQ.5.0:  𝑞 in Hocket-Sherby hardening law 
HTFLAG 
Heat treatment flag : 
HTFLAG.EQ.0:  Preforming stage 
HTFLAG.EQ.1:  Heat treatment stage 
HTFLAG.EQ.2:  Postforming stage 
HTA 
HTB 
HTC 
HTD 
Load curve/Table ID for postforming parameter A 
Load curve/Table ID for postforming parameter B 
Load curve/Table ID for postforming parameter C 
Load curve/Table ID for postforming parameter D 
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3 
D1, D2, D3 
Components of vector 𝐝 for AOPT = 2 
USRFAIL 
User defined failure flag  
EQ.0: no user subroutine is called 
EQ.1: user subroutine matusr_24 in dyn21.f is called 
Remarks: 
1.  Strain rate is accounted for using the Cowper and Symonds model which scales 
the yield stress with the factor 
1 + (
𝑝⁄
)
𝜀̇
where 𝜀̇ is the strain rate.   To ignore strain rate effects set both C and P to zero.
2.  The yield condition for this material can be written 
𝑓 (σ,α, 𝜀𝑝) = 𝜎eff(𝜎𝑥𝑥 − 2𝛼𝑥𝑥 − 𝛼𝑦𝑦, 𝜎𝑦𝑦 − 2𝛼𝑦𝑦 − 𝛼𝑥𝑥, 𝜎𝑥𝑦 − 𝛼𝑥𝑦) − 𝜎𝑌
𝑡 (𝜀𝑝, 𝜀̇𝑝, 𝛽) ≤ 0 
where 
𝜎eff(𝑠𝑥𝑥, 𝑠𝑦𝑦, 𝑠𝑥𝑦) = [
1/𝑎
(𝜑′ + 𝜑′′)]
𝜑′ = ∣𝑋′1 − 𝑋′2∣𝑎 
𝜑′′ = ∣2𝑋1
′′ + X2
′′∣𝑎 + ∣X1
′′ + 2X2
′′∣𝑎. 
The 𝑋′𝑖 and 𝑋′′𝑖 are eigenvalues of 𝑋′𝑖𝑗  and 𝑋′′𝑖𝑗 and are given by  
and  
′ =
𝑋1
′ =
𝑋2
′′ =
𝑋1
′′ =
𝑋2
(𝑋11
′ + 𝑋22
′ + √(𝑋11
′ − 𝑋22
′ )2 + 4𝑋12
′ 2) 
(𝑋11
′ + 𝑋22
′ − √(𝑋11
′ − 𝑋22
′ )2 + 4𝑋12
′ 2) 
(𝑋11
′′ + 𝑋22
′′ + √(𝑋11
′′ − 𝑋22
′′ )2 + 4𝑋12
′′ 2) 
(𝑋11
′′ + 𝑋22
′′ − √(𝑋11
′′ − 𝑋22
′′ )2 + 4𝑋12
′′ 2) 
respectively.  The 𝑋′𝑖𝑗  and 𝑋′′𝑖𝑗 are given by 
′
𝑋11
⎟⎟⎟⎞
′
𝑋22
′ ⎠
𝑋12
′′
𝑋11
⎟⎟⎟⎞
′′
𝑋22
′′ ⎠
𝑋12
⎜⎜⎜⎛
⎝
⎜⎜⎜⎛
⎝
=
=
′
𝐿11
′
𝐿21
⎜⎜⎜⎛
⎝
′′
𝐿11
′′
𝐿21
⎜⎜⎜⎛
⎝
′
𝐿12
′
𝐿22
′′
𝐿12
′′
𝐿22
⎟⎟⎟⎞
′ ⎠
𝐿33
⎟⎟⎟⎞
′′ ⎠
𝐿33
𝑠𝑥𝑥
⎟⎞ 
𝑠𝑦𝑦
𝑠𝑥𝑦⎠
⎜⎛
⎝
𝑠𝑥𝑥
⎟⎞ 
𝑠𝑦𝑦
𝑠𝑥𝑦⎠
⎜⎛
⎝
Where, 
⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞
′
𝐿11
′
𝐿12
′
𝐿21
′
𝐿22
′ ⎠
𝐿33
′′
𝐿11
′′
𝐿12
′′
𝐿21
′′
𝐿22
′′ ⎠
𝐿33
⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞
⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛
⎝
⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛
⎝
=
−1
0 −1
⎜⎜⎜⎜⎜⎜⎜⎛
⎝
⎟⎟⎟⎟⎟⎟⎟⎞
3⎠
𝛼1
⎟⎞ 
𝛼2
𝛼7⎠
⎜⎛
⎝
=
⎜⎜⎜⎜⎜⎜⎜⎛
⎝
−2
1 −4 −4
4 −4 −4
8 −2
2 −2
−2
⎟⎟⎟⎟⎟⎟⎟⎞
9⎠
⎟⎟⎟⎟⎟⎟⎟⎞
𝛼3
𝛼4
𝛼5
𝛼6
𝛼8⎠
⎜⎜⎜⎜⎜⎜⎜⎛
⎝
The  parameters  𝛼1  to  𝛼8  are  the  parameters  that  determines  the  shape  of  the 
yield surface.
The  material  parameters  can  be  determined  from  three  uniaxial  tests  and  a 
more general test.  From the uniaxial tests the yield stress and R-values are used 
and from the general test an arbitrary point on the yield surface is used given 
by the stress components in the material system as 
𝛔 =
𝜎𝑥𝑥
⎟⎟⎞ 
𝜎𝑦𝑦
𝜎𝑥𝑦⎠
⎜⎜⎛
⎝
together  with  a  tangent  of  the  yield  surface  in  that  particular  point.    For  the 
latter the tangential direction should be determined so that 
𝑑𝑥𝑥𝜀̇𝑥𝑥
𝑝 + 𝑑𝑦𝑦𝜀̇𝑦𝑦
𝑝 + 2𝑑𝑥𝑦𝜀̇𝑥𝑦
𝑝 = 0 
The biaxial data can be set to zero in the input deck for LS-DYNA to just fit the 
uniaxial data. 
3.  A kinematic hardening model is implemented following the works of Chaboche 
and  Roussilier.    A  back  stress  α  is  introduced  such  that  the  effective  stress  is 
computed as 
𝜎eff = 𝜎eff(𝜎11 − 2𝛼11 − 𝛼22, 𝜎22 − 2𝛼22 − 𝛼11, 𝜎12 − 𝛼12) 
The back stress is the sum of up to four terms according to 
𝛼𝑖𝑗 = ∑ 𝛼𝑖𝑗
𝑘=1
and the evolution of each back stress component is as follows 
𝛿𝛼𝑖𝑗
𝑘 = 𝐶𝑘 (𝑎𝑘
𝑠𝑖𝑗
𝜎eff
− 𝛼𝑖𝑗
𝑘 ) 𝛿𝜀𝑝 
where 𝐶𝑘 and 𝑎𝑘 are material parameters, 𝑠𝑖𝑗 is the deviatoric stress tensor, 𝜎eff is 
the  effective  stress  and  𝜀𝑝  is  the  effective  plastic  strain.    The  yield  condition  is 
for this case modified according to 
𝑓 (𝛔, 𝛂, 𝜀𝑝)
= 𝜎eff(𝜎𝑥𝑥 − 2𝛼𝑥𝑥 − 𝛼𝑦𝑦, 𝜎𝑦𝑦 − 2𝛼𝑦𝑦 − 𝛼𝑥𝑥, 𝜎𝑥𝑦 − 𝛼𝑥𝑦)
−   {𝜎𝑌
𝑡 (𝜀𝑝, 𝜀̇𝑝, 0) − ∑ 𝑎𝑘[1 − exp(−𝐶𝑘𝜀𝑝) ]
} ≤ 0 
𝑘=1
in order to get the expected stress strain response for uniaxial stress. 
4.  The Hansel hardening law is the same as in material 113 but is repeated here for 
the sake of convenience.  
The  hardening  is  temperature  dependent  and  therefore  this  material  model 
must  be  run  either  in  a  coupled  thermo-mechanical  solution,  using  prescribed
temperatures or using the adiabatic temperature calculation option.  Setting the 
parameter CP to the specific heat Cp of the material activates the adiabatic tem-
perature calculation that calculates the temperature rate from the equation  
𝜎𝐢𝐣𝐷𝑖𝑗
𝜌𝐶𝑝
, 
𝑇̇ = ∑
𝑖,𝑗
where 𝛔: 𝐃𝑝 (the numerator) is the plastically dissipated heat.  Using the Kelvin 
scale  is  recommended,  even  though  other  scales  may  be  used  without  prob-
lems. 
The hardening behaviour is described by the following equations.  The marten-
site rate equation is 
∂𝑉𝑚
∂𝜀̅𝑝
⎧0
{{
⎨
{{
⎩
=
𝑉𝑚
𝑝 (
1 − 𝑉𝑚
𝑉𝑚
)
𝐵+1
𝐵 [1 − tanh(𝐶 + D × 𝑇)]
𝜀 < 𝐸0(mart)
exp (
𝑇 − 𝑇𝐴0
) 𝜀̅𝑝 ≥ 𝐸0(mart)
Where 
𝜀̅𝑝 = effective plastic strain 
𝑇 = temperature 
The martensite fraction is integrated from the above rate equation: 
𝑉𝑚 = ∫
∂𝑉𝑚
∂𝜀̅𝑝
𝑑𝜀̅𝑝. 
It  always  holds  that  0.0 < 𝑉𝑀 < 1.0.  The  initial  martensite  content  is  Vm0  and 
must be greater than zero and less than 1.0.  Note that 𝑉𝑀0 is not used during a 
restart  or  when  initializing  the  Vm  history  variable  using  *INITIAL_STRESS_-
SHELL. 
The yield stress σy is 
𝜎𝑦 = {𝐵𝐻𝑆 − (𝐵𝐻𝑆 − 𝐴𝐻𝑆)exp(−𝑚[𝜀̅𝑝 + 𝜀0]𝑛)}(𝐾1 + 𝐾2𝑇) + Δ𝐻𝛾→𝛼′𝑉𝑚. 
The parameters p and B should fulfill the following condition 
1 + 𝐵
< 𝑝, 
if not fulfilled then the martensite rate will approach infinity as 𝑉𝑚 approaches 
zero.  Setting  the  parameter 𝜀0  larger  than  zero,  typical  range  0.001-0.02  is  rec-
ommended.  A part from the effective true strain a few additional history varia-
bles are output, see below.
History variables that are output for post-processing: 
Variable Description 
24  Yield  stress  of  material  at  temperature  TREF.    Useful  to  evaluate  the 
strength of the material after e.g., a simulated forming operation. 
25  Volume fraction martensite, Vm 
26  CP.EQ.0.0: Not used 
CP.GT.0.0: Temperature from adiabatic temperature calculation. 
5.  Heat  treatment  for  increasing  the  formability  of  prestrained  aluminum  sheets 
can  be  simulated  through  the  use  of  HTFLAG,  where  the  intention  is  to  run  a 
forming  simulation  in  steps  involving  preforming,  springback,  heat  treatment 
and postforming.  In each step the history is transferred to the next via the use 
of  dynain  .    The  first  two  steps  are  per-
formed  with  HTFLAG = 0  according  to  standard  procedures,  resulting  in  a 
0corresponding to the prestrain.  The heat treatment step is 
plastic strain field 𝜀𝑝
performed  using  HTFLAG = 1  in  a  coupled  thermomechanical  simulation, 
where  the  blank  is  heated.    The  coupling  between  thermal  and  mechanical  is 
only  that  the  maximum  temperature  𝑇0  is  stored  as  a  history  variable  in  the 
material model, this corresponding to the heat treatment temperature.  Here it 
is important to export all history variables to the dynein file for the postforming 
step.    In  the  final  postforming  step,  HTFLAG = 2,  the  yield  stress  is  then  aug-
mented by the Hocket-Sherby like term 
0)
Δ𝜎 = 𝑏 − (𝑏 − 𝑎)exp[−𝑐(𝜀𝑝 − 𝜀𝑝
] 
where a, b, c and d are given as tables as functions of the heat treatment temper-
ature 𝑇0 and prestrain 𝜀𝑝
0. That is, in the table definitions each load curve corre-
sponds to a given prestrain and the load curve value is with respect to the heat 
treatment temperature, 
𝑎 = 𝑎(𝑇0, 𝜀𝑝
𝑑 = 𝑑(𝑇0, 𝜀𝑝
𝑏 = 𝑏(𝑇0, 𝜀𝑝
𝑐 = 𝑐(𝑇0, 𝜀𝑝
0)     
0),
0),
0),
The effect of heat treatment is that the material strength decreases but harden-
ing increases, thus typically, 
𝑎 ≤ 0,
𝑏 ≥ 𝑎,
𝑐 > 0,
𝑑 > 0.
*MAT_134 
This  is  Material  Type  134.    The  viscoelastic  fabric  model  is  a  variation  on  the  general 
viscoelastic  model  of  material  76.    This  model  is  valid  for  3  and  4  node  membrane 
elements only and is strongly recommended for modeling isotropic viscoelastic fabrics 
where wrinkling may be a problem.  For thin fabrics, buckling can result in an inability 
to  support  compressive  stresses;  thus,  a  flag  is  included  for  this  option.    If  bending 
stresses are important use a shell formulation with model 76. 
  Card 1 
1 
Variable 
MID 
Type 
I 
2 
RO 
F 
3 
4 
5 
6 
BULK 
F 
8 
7 
CSE 
F 
If fitting is done from a relaxation curve, specify fitting parameters on card 2, otherwise
if constants are set on Viscoelastic Constant Cards LEAVE THIS CARD BLANK. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
NT 
BSTART 
TRAMP 
LCIDK 
NTK 
BSTARTK  TRAMPK 
Type 
F 
I 
F 
F 
F 
I 
F 
F 
Viscoelastic Constant Cards.  Up to 6 cards may be input.  A keyword card (with a 
“*” in column 1) terminates this input if less than 6 cards are used.  These cards are not 
needed if relaxation data is defined.  The number of terms for the shear behavior may 
differ from that for the bulk behavior: simply insert zero if a term is not included. 
  Card 3 
Variable 
Type 
1 
GI 
F 
2 
BETAI 
F 
3 
KI 
F 
4 
5 
6 
7 
8 
BETAKI 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
Material identification.  A unique number must be specified. 
Mass density.
BULK 
*MAT_VISCOELASTIC_FABRIC 
DESCRIPTION
Elastic  constant  bulk  modulus. 
is
viscoelastic, then this modulus is used in determining the contact
interface stiffness only. 
  If  the  bulk  behavior 
CSE 
Compressive stress flag (default = 0.0). 
EQ.0.0: don’t eliminate compressive stresses 
EQ.1.0: eliminate compressive stresses 
LCID 
NT 
BSTART 
Load  curve  ID  if  constants,  Gi,  and  βi  are  determined  via  a  least 
squares fit.  This relaxation curve is shown below. 
Number of terms in shear fit.  If zero the default is 6.  Currently,
the maximum number is set to 6. 
In the fit, β1  is set to zero, β2  is set to BSTART, β3  is 10 times β2, 
β4 is 10 times β3 , and so on.  If zero, BSTART = 0.01. 
TRAMP 
Optional ramp time for loading. 
LCIDK 
Load  curve  ID  for  bulk  behavior  if  constants,  Ki,  and  βκi    are 
determined via a least squares fit.  This relaxation curve is shown
below. 
NTK 
Number  of  terms  desired  in  bulk  fit.    If  zero  the  default  is  6.
Currently, the maximum number is set to 6. 
BSTARTK 
In  the  fit,  βκ1    is  set  to  zero,  βκ2    is  set  to  BSTARTK,  βκ3    is  10 
times  βκ2,  βκ4 
  If  zero, 
BSTARTK = 0.01. 
is  10  times  βκ3 
,  and  so  on. 
TRAMPK 
Optional ramp time for bulk loading. 
GI 
Optional shear relaxation modulus for the ith term 
BETAI 
Optional shear decay constant for the ith term 
KI 
Optional bulk relaxation modulus for the ith term 
BETAKI 
Optional bulk decay constant for the ith term
Remarks: 
Rate  effects  are  taken  into  accounted  through  linear  viscoelasticity  by  a  convolution 
integral of the form: 
𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙
(𝑡 − 𝜏)
∂𝜀𝑘𝑙
∂𝜏
𝑑𝜏 
where  𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)    is  the  relaxation  function.If  we  wish  to  include  only  simple  rate 
effects  for  the  deviatoric  stresses,  the  relaxation  function  is  represented  by  six  terms 
from the Prony series: 
𝑔(𝑡) = ∑ 𝐺𝑚
𝑚=1
𝑒−𝛽𝑚 𝑡 
We  characterize  this  in  the  input  by  shear  modulii,  𝐺𝑖,  and  decay  constants,  𝛽𝑖.    An 
arbitrary number of terms, up to 6, may be used when applying the viscoelastic model.  
For volumetric relaxation, the relaxation function is also represented by the Prony series 
in terms of bulk modulii: 
𝑘(𝑡) = ∑ 𝐾𝑚
𝑚=1
𝑒−𝛽𝑘𝑚 𝑡
σ∕ε
TRAMP
10n
10n+1 10n+2 10n+3
time
optional ramp time for loading
Figure M134-1.  Stress Relaxation curve. 
For an example of a stress relaxation curve see Figure M134-1.  This curve defines stress 
versus  time  where  time  is  defined  on  a  logarithmic  scale.    For  best  results,  the  points 
defined  in  the  load  curve  should  be  equally  spaced  on  the  logarithmic  scale.  
Furthermore, the load curve should be smooth and defined in the positive quadrant.  If 
nonphysical  values  are  determined  by  least  squares  fit,  LS-DYNA  will  terminate  with 
an  error  message  after  the  initialization  phase  is  completed.    If  the  ramp  time  for 
loading is included, then the relaxation which occurs during the loading phase is taken 
into account.  This effect may or may not be important.
*MAT_135 
This is material type 135.  This anisotropic-viscoplastic material model adopts two yield 
criteria  for  metals  with  orthotropic  anisotropy  proposed  by  Barlat  and  Lian  [1989] 
(Weak Texture Model) and Aretz [2004] (Strong Texture Model). 
5 
6 
7 
8 
NUMFI 
EPSC 
WC 
TAUC 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
E 
F 
3 
4 
PR 
F 
4 
F 
5 
Variable 
SIGMA0 
QR1 
CR1 
QR2 
CR2 
Type 
F 
F 
F 
F 
F 
YLD2003 Card.  This card 3 format is used when FLG = 0. 
  Card 3 
Variable 
1 
A1 
Type 
F 
2 
A2 
F 
3 
A3 
F 
4 
A4 
F 
5 
A5 
F 
F 
6 
K 
F 
6 
A6 
F 
F 
7 
LC 
F 
7 
A7 
F 
F 
8 
FLG 
F 
8 
A8 
F 
Yield Surface Card.  This card 3 format is used when FLG = 1. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
S00 
S45 
S90 
SBB 
R00 
R45 
R90 
RBB 
Type 
F 
F 
F 
F 
F 
F 
F
YLD89 Card.  This card 3 format used when FLG = 2. 
5 
6 
7 
8 
  Card 3 
Variable 
Type 
1 
A 
F 
  Card 4 
1 
2 
C 
F 
2 
3 
H 
F 
3 
4 
P 
F 
4 
5 
Variable 
QX1 
CX1 
QX2 
CX2 
EDOT 
7 
8 
EMIN 
S100 
F 
7 
F 
8 
7 
8 
7 
8 
6 
M 
F 
6 
6 
A3 
F 
6 
D3 
F 
F 
3 
3 
ZP 
F 
3 
V3 
F 
F 
4 
4 
A1 
F 
4 
D1 
F 
F 
5 
5 
A2 
F 
5 
D2 
F 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
LS-DYNA R10.0 
Type 
F 
  Card 5 
1 
F 
2 
Variable 
AOPT 
BETA 
Type 
F 
F 
2 
YP 
F 
2 
V2 
F 
  Card 6 
Variable 
1 
XP 
Type 
F 
  Card 7 
Variable 
1 
V1 
Type 
F 
  VARIABLE
VARIABLE   
DESCRIPTION
RO 
E 
PR 
NUMFI 
EPSC 
WC 
TAUC 
Mass density 
Young’s modulus 
Poisson’s ratio 
Number  of  through  thickness  integration  points  that  must  fail
before the element is deleted (remember to change this number if 
switching between full and reduced integration type of elements).
Critical  value 𝜀𝑡𝐶  of  the  plastic  thickness  strain  (used  in  the  CTS
fracture criterion).   
Critical value 𝑊𝑐 for the Cockcroft-Latham fracture criterion 
Critical value 𝜏𝑐 for the Bressan-Williams shear fracture criterion 
SIGMA0 
Initial mean value of yield stress 𝜎0:  
GT.0.0:  Constant value, 
LT.0.0:  Load curve ID = -SIGMA0 which defines yield stress as 
a  function  of  plastic  strain.    Hardening  parameters
QR1, CR1, QR2, and CR2 are ignored in that case. 
QR1 
CR1 
QR2 
CR2 
K 
LC 
A1 
A2 
A3 
Isotropic hardening parameter 𝑄𝑅1 
Isotropic hardening parameter 𝐶𝑅1 
Isotropic hardening parameter 𝑄𝑅2 
Isotropic hardening parameter 𝐶𝑅2 
𝑘 equals half YLD2003 exponent 𝑚.  Recommended value for FCC 
materials is 𝑚 = 8, i.e. 𝑘 = 4. 
First  load  curve  number  for  process  effects,  i.e.    the  load  curve
describing the relation between the pre-strain and the yield stress 
𝜎0.    Similar  curves  for  𝑄𝑅1,  𝐶𝑅1,  𝑄𝑅2,  𝐶𝑅2,  and  𝑊𝑐  must  follow 
consecutively from this number. 
Yld2003 parameter 𝑎1 
Yld2003 parameter 𝑎2 
Yld2003 parameter 𝑎3
*MAT_WTM_STM 
DESCRIPTION
A4 
A5 
A6 
A7 
A8 
S00 
S45 
S90 
SBB 
R00 
R45 
R90 
RBB 
A 
C 
H 
P 
QX1 
CX1 
QX2 
CX2 
Yld2003 parameter 𝑎4 
Yld2003 parameter 𝑎5 
Yld2003 parameter 𝑎6 
Yld2003 parameter 𝑎7 
Yld2003 parameter 𝑎8 
Yield stress in 0° direction 
Yield stress in 45° direction 
Yield stress in 90° direction 
Balanced biaxial flow stress 
R-ratio in 0° direction 
R-ratio in 45° direction 
R-ratio in 90° direction 
Balance biaxial flow ratio 
YLD89 parameter a 
YLD89 parameter c 
YLD89 parameter h 
YLD89 parameter p 
Kinematic hardening parameter 𝑄𝑥1 
Kinematic hardening parameter 𝐶𝑥1 
Kinematic hardening parameter 𝑄𝑥2 
Kinematic hardening parameter 𝐶𝑥2 
EDOT 
Strain rate parameter 𝜀̇0 
M 
Strain rate parameter 𝑚
EMIN 
*MAT_135 
DESCRIPTION
Lower  limit  of  the  isotropic  hardening  rate  𝑑𝑅
𝑑𝜀̅.    This  feature  is 
included  to  model  a  non-zero  and  linear/exponential  isotropic 
work  hardening  rate  at  large values  of  effective  plastic  strain.   If
the isotropic work hardening rate predicted by the utilized Voce-
type  work  hardening  rule  falls  below  the  specified  value  it  is 
substituted  by  the  prescribed  value  or  switched  to  a  power-law 
hardening  if  S100.NE.0.    This  option  should  be  considered  for
problems  involving  extensive  plastic  deformations.    If  process
dependent  material  characteristics  are  prescribed,  i.e.    if  LC  .GT. 
0  the  same  minimum  tangent  modulus  is  assumed  for  all  the
prescribed  work  hardening  curves.    If  instead  EMIN.LT.0  then  –
EMIN  defines  the  plastic  strain  value  at  which  the  linear  or
power-law hardening approximation commences. 
S100 
AOPT 
Yield  stress  at  100%  strain  for  using  a  power-law  approximation 
beyond the strain defined by EMIN. 
Material  axes  option  : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES,  and  then  rotated  about  the  shell  ele-
ment normal by an angle BETA. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the
element normal. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID 
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later.. 
BETA 
Material angle in degrees for AOPT = 0 or 3, may be overwritten 
on the element card, see *ELEMENT_SHELL_BETA. 
XP YP ZP 
Coordinates of point p for AOPT = 1.
*MAT_WTM_STM 
DESCRIPTION
A1 A2 A3 
Components of vector a for AOPT = 2. 
V1 V2 V3 
Components of vector v for AOPT = 3 
D1 D2 D3 
Components of vector d for AOPT = 2. 
Remarks: 
If  FLG = 1,  i.e.    if  the  yield  surface  parameters  𝑎1−𝑎8  are  identified  on  the  basis  of 
prescribed  material  data  internally  in  the  material  routine,  files  with  point  data  for 
plotting of the identified yield surface, along with the predicted directional variation of 
the  yield  stress  and  plastic  flow  are  generated  in  the  directory  where  the  LS-DYNA 
analysis is run.  Four different files are generated for each specified material. 
These files are named according to the scheme: 
1.  Contour_1# 
2.  Contour_2# 
3.  Contour_3# 
4.  R_and_S# 
Where # is a value starting at 1. 
The  three  first  files  contain  contour  data  for  plotting  of  the  yield  surface  as  shown  in 
Figure M135-2.  To generate these plots a suitable plotting program should be adopted 
and for each file/plot, column A should be plotted vs.  columns B.  For a more detailed 
description  of  these  plots  it  is  referred  to  References.    Figure  M135-3  further  shows  a 
plot  generated  from  the  final  file  named  ‘R_and_S#’  showing  the  directional 
dependency  of  the  normalized  yield  stress  (column  A  vs.    B)  and  plastic  strain  ratio 
(column B vs.  C). 
The yield condition for this material can be written 
𝑡(σ, α, 𝜀𝑝, 𝜀̇𝑝) = 𝜎eff(σ, α) − 𝜎𝑌(𝜀𝑝, 𝜀̇𝑝) 
where  
𝜎𝑌 = [𝜎0 + 𝑅(𝜀𝑝)] (1 +
)
𝜀̇𝑝
𝜀̇0
where the isotropic hardening reads 
𝑅(𝜀̇𝑝) = 𝑄𝑅1[1 − exp(−𝐶𝑅1𝜀𝑝)] + 𝑄𝑅2[1 − exp(−𝐶𝑅2𝜀𝑝)].
For the Weak Texture Model the yield function is defined as  
𝜎eff = [
{𝑎(𝑘1 + 𝑘2)𝑚 + 𝑎(𝑘1 − 𝑘2)𝑚 + 𝐶(2𝑘2)𝑚}]
where  
𝑘1 =
𝜎𝑥 + ℎ  𝜎𝑦
√
√√
⎷
(
𝜎𝑥 + ℎ  𝜎𝑦
)
𝑘2 =
+ (𝑟  𝜎𝑥𝑦)
. 
For the Strong Texture Model the yield function is defined as 
𝜎eff = {
where 
[(𝜎+
′ )𝑚 + (𝜎−
′ )𝑚 + (𝜎+
′′ − 𝜎−
′′)𝑚]}
′ =
σ±
𝑎8𝜎𝑥 + 𝑎1𝜎𝑦
± √(
𝑎2𝜎𝑥 − 𝑎3𝜎𝑦
)
+ 𝑎4
2𝜎𝑥𝑦
2  
′′ =
σ±
𝜎𝑥 + 𝜎𝑦
± √(
𝑎5𝜎𝑥 − 𝑎6𝜎𝑦
)
+ 𝑎7
2  𝜎𝑥𝑦. 
Kinematic hardening can be included by  
α = ∑ α𝑅
𝑅=1
where  each  of  the  kinematic  hardening  variables  𝛼𝑅  is  independent  and  obeys  a 
nonlinear evolutionary equation in the form 
where the effective stress 𝜎̅̅̅̅̅ is defined as  
α̇𝑅 = 𝐶𝛼𝑖 (𝑄𝛼𝑖
− α𝑅) 𝜀̇𝑝 
where 
𝜎̅̅̅̅̅ = 𝜎eff(τ) 
τ = σ − α. 
Critical thickness strain failure in a layer is assumed to occur when 
𝜀𝑡 ≤ 𝜀𝑡𝑐 
where 𝜀𝑡𝑐 is a material parameter.  It should be noted that 𝜀𝑡𝑐 is a negative number (i.e.  
failure is assumed to occur only in the case of thinning). 
Cockcraft and Latham fracture is assumed to occur when
where 𝜎1 is the maximum principal stress and 𝑊𝐶 is a material parameter. 
𝑊 = ∫ max(𝜎1, 0)𝑑𝜀𝑝 ≥ 𝑊𝐶 
History 
Variable 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
11 
12 
13 
14 
Description 
Isotropic hardening value 𝑅1 
Isotropic hardening value 𝑅2 
Increment in effective plastic strain Δ𝜀̅ 
Not defined, for internal use in the material model 
Not defined, for internal use in the material model 
Not defined, for internal use in the material model 
Failure in integration point 
EQ.0: No failure 
EQ.1: Failure due to EPSC, i.e. 𝜀𝑡 ≥ 𝜀𝑡𝑐. 
EQ.2: Failure due to WC, i.e. 𝑊 ≥ 𝑊𝑐. 
EQ.3: Failure due to TAUC, i.e. 𝜏 ≥ 𝜏𝑐 
Sum  of 
incremental  strain 
𝜀𝑥𝑥 = ∑ Δ𝜀𝑥𝑥 
Sum  of 
𝜀𝑦𝑦 = ∑ Δ𝜀𝑦𝑦 
incremental  strain 
in 
in 
local  element  x-direction: 
local  element  y-direction: 
Value of theh Cockcroft-Latham failure parameter 𝑊 = ∑ 𝜎1Δ𝑝 
Plastic strain component in thickness direction 𝜀𝑡 
Mean value of increments in plastic strain through the thickness 
(For  use  with  the  non-local  instability  criterion.    Note  that 
constant  lamella  thickness  is  assumed  and  the  instability 
criterion can give unrealistic results if used with a user-defined 
integration rule with varying lamella thickness.) 
Not defined, for internal use in the material model 
Nonlocal value 𝜌 =
Δ𝜀3
Ω 
Δ𝜀3
Table M135-1.
1.5
0.5
-0.5
-1
-1.5
-1.5
-1
-0.5
1.5
0.75
xy
-0.75
-1.5
0.5
1.5
-1.5
-0.75
(A)
1.5
0.75
xy
-0.75
-1.5
0.75
1.5
√2(σ
x+σ
2σ
y)
(B)
0.75
1.5
-1.5
-0.75
√2(σ
x-σ
2σ
y)
(C)
Figure M135-2.  Contour plots of the yield surface generated from the files (a)
‘Contour_1<#>’, (b) Contour_2<#>’, and (c) ‘Contour_3<#>’.
1.1
1.05
σα
0.95
1.6
1.2
0.8
0.4
Rα
0.9
30
α [deg]
60
90
Figure M135-3.  Predicted directional variation of the yield stress and plastic
flow generated from the file ‘R_and_S<#>’.
*MAT_135_PLC 
This is Material Type 135.  This anisotropic material adopts the yield criteria proposed 
by Aretz [2004].  The material strength is defined by McCormick’s constitutive relation 
for materials exhibiting negative steady-state Strain Rate Sensitivity (SRS).  McCormick 
[1998] and Zhang, McCormick and Estrin [2001]. 
5 
6 
7 
8 
NUMFI 
EPSC 
WC 
TAUC 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
E 
F 
3 
4 
PR 
F 
4 
F 
5 
Variable 
SIGMA0 
QR1 
CR1 
QR2 
CR2 
Type 
F 
F 
F 
F 
F 
  Card 3 
Variable 
1 
A1 
Type 
F 
  Card 4 
Variable 
Type 
1 
S 
F 
2 
A2 
F 
2 
H 
F 
3 
A3 
F 
3 
4 
A4 
F 
4 
5 
A5 
F 
5 
OMEGA 
TD 
ALPHA 
EPS0 
F 
F 
F 
F 
F 
6 
K 
F 
6 
A6 
F 
6 
F 
7 
7 
A7 
F 
7 
F 
8 
8 
A8 
F
Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
AOPT 
BETA 
Type 
F 
F 
  Card 6 
Variable 
1 
XP 
Type 
F 
  Card 7 
Variable 
1 
V1 
Type 
F 
2 
YP 
F 
2 
V2 
F 
3 
ZP 
F 
3 
V3 
F 
4 
A1 
F 
4 
D1 
F 
5 
A2 
F 
5 
D2 
F 
6 
A3 
F 
6 
D3 
F 
7 
8 
7 
8 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
NUMFI 
EPSC 
WC 
TAUC 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s modulus 
Poisson’s ratio 
Number  of  through  thickness  integration  points  that  must  fail
before the element is deleted (remember to change this number if
switching between full and reduced integration type of elements).
Critical value 𝜀𝑡𝐶 of the plastic thickness strain. 
Critical value 𝑊𝑐 for the Cockcroft-Latham fracture criterion. 
Critical value 𝜏𝑐 for the shear fracture criterion. 
SIGMA0 
Initial yield stress 𝜎0
VARIABLE   
DESCRIPTION
QR1 
CR1 
QR2 
CR2 
K 
A1 
A2 
A3 
A4 
A5 
A6 
A7 
A8 
S 
H 
Isotropic hardening parameter, 𝑄𝑅1 
Isotropic hardening parameter, 𝐶𝑅1 
Isotropic hardening parameter, 𝑄𝑅2 
Isotropic hardening parameter, 𝐶𝑅2 
k equals half the exponent m for the yield criterion 
Yld2003 parameter, 𝑎1 
Yld2003 parameter, 𝑎2 
Yld2003 parameter, 𝑎3 
Yld2003 parameter, 𝑎4 
Yld2003 parameter, 𝑎5 
Yld2003 parameter, 𝑎6 
Yld2003 parameter, 𝑎7 
Yld2003 parameter, 𝑎8 
Dynamic strain aging parameter, S. 
Dynamic strain aging parameter, H. 
OMEGA 
Dynamic strain aging parameter, Ω. 
TD 
Dynamic strain aging parameter, 𝑡𝑑. 
ALPHA 
Dynamic strain aging parameter, 𝛼. 
EPS0 
AOPT 
Dynamic strain aging parameter, 𝜀̇0. 
Material  axes  option   
EQ.0.0: Locally  orthotropic  with  material  axes  determined  by
element  nodes  as  shown  in  Figure  M2-1,  and  then  ro-
tated  about  the  shell  element  normal  by  the  angle  BE-
TA.  Nodes 1, 2 and 4 of an element are identical to the
nodes used for the definition of a coordinate system as
by *DEFINE_COORDINATE_NODES.
VARIABLE   
DESCRIPTION
EQ.2.0: Globally orthotropic with material axes determined by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: Locally  orthotropic  material  axes  determined  by
offsetting the material axes by an angle, BETA, from a
line determined by taking the cross product of the vec-
tor v with the normal to the plane of the element. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
BETA 
Material angle in degrees for AOPT = 0 and 3, may be overwritten 
on the element card, see *ELEMENT_SHELL_BETA.   
XP, YP, ZP 
Coordinates of point p for AOPT = 1. 
A1, A2, A3 
Components of vector a for AOPT = 2. 
V1, V2, V3 
Components of vector v for AOPT = 3. 
D1, D2, D3 
Components of vector d for AOPT = 2. 
Remarks: 
The yield function is defined as 
𝑓 = 𝑓 ̅(σ) − [𝜎𝑌(𝑡𝑎) + 𝑅(𝜀𝑝) + 𝜎𝑣(𝜀̇𝑝)] 
where the equivalent stress 𝜎eq is defined as by an anisotropic yield criterion 
𝜎eq = [
(∣𝜎′1∣𝑚 + ∣𝜎′2∣𝑚 + ∣𝜎′′1 − 𝜎′′2∣)]
where 
and 
{
𝜎′1
𝜎′2
} =
𝑎8𝜎𝑥𝑥 + 𝑎1𝜎𝑦𝑦
± √(
𝑎2𝜎𝑥𝑥 − 𝑎3𝜎𝑦𝑦
)
+ 𝑎4
2𝜎𝑥𝑦
2  
𝜎′′1
{
𝜎′′2
} =
𝜎𝑥𝑥 + 𝜎𝑦𝑦
± √(
𝑎5𝜎𝑥𝑥 − 𝑎6𝜎𝑦𝑦
)
+ 𝑎7
2𝜎𝑥𝑦
The strain hardening function R is defined  by the extended Voce law 
𝑅(𝜀𝑝) = ∑ 𝑄𝑅𝑖(1 − exp(−𝐶𝑅𝑖𝜀𝑝))
𝑖=1
where  𝜀𝑝  is  the  effective  (or  accumulated)  plastic  strain,  and  𝑄𝑅𝑖and  𝐶𝑅𝑖  are  strain 
hardening parameters. 
Viscous stress 𝜎𝑣 is given by 
𝜎𝑣 = (𝜀̇𝑝) = 𝑠 ln (1 +
𝜀̇𝑝
𝜀̇0
) 
where S  represents  the  instantaneous  strain  rate  sensitivity  (SRS)  and  𝜀̇0  is  a  reference 
strain  rate.   In  this  model  the  yield  strength,  including  the  contribution  from  dynamic 
strain aging (DSA) is defined as 
𝜎𝑌(𝑡𝑎) = 𝜎0 + SH [1 − exp {− (
)
𝑡𝑎
𝑡𝑑
}] 
where 𝜎0is the yield strength for vanishing average waiting time, 𝑡𝑎, i.e.  at high strain 
rates,  and  H,  𝛼and  𝑡𝑑  are  material  constants  linked  to  dynamic  strain  aging.    It  is 
noteworthy that 𝜎𝑌 is an increasing function of 𝑡𝑎. The average waiting time is defined 
by the evolution equation 
𝑡 ̇𝑎 = 1 −
𝑡𝑎
𝑡𝑎,𝑠𝑠
where the quasi-steady waiting time 𝑡𝑎,𝑠𝑠 is given as 
𝑡𝑎,𝑠𝑠 =
𝜀̇𝑝 
where Ω is the strain produced by all mobile  dislocations moving to the next obstacle 
on their path.
*MAT_CORUS_VEGTER 
This is Material Type 136, a plane stress orthotropic material model for metal forming.  
Yield surface construction is based on the interpolation by second-order Bezier curves, 
and model parameters are determined directly from a set of mechanical tests conducted 
for a number of directions.  For each direction, four mechanical tests are carried out: a 
uniaxial,  an  equi-biaxial,  a  plane  strain  tensile  test  and  a  shear  test.    These  test  results 
are used to determine the coefficients of the Fourier directional dependency field.  For a 
more detailed description please see Vegter and Boogaard [2006]. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
E 
F 
3 
4 
PR 
F 
4 
5 
N 
F 
5 
Variable 
SYS 
SIP 
SHS 
SHL 
ESH 
Type 
F 
  Card 3 
1 
Variable 
AOPT 
Type 
  Card 4 
Variable 
1 
XP 
Type 
F 
F 
2 
2 
YP 
F 
F 
3 
3 
ZP 
F 
F 
4 
4 
A1 
F 
F 
5 
5 
A2 
F 
6 
FBI 
F 
6 
E0 
F 
6 
6 
A3 
F 
7 
8 
RBI0 
LCID 
F 
7 
F 
8 
ALPHA 
LCID2 
F 
7 
F 
8 
7
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
*MAT_136 
7 
8 
BETA 
F 
Experimental Data Cards.  The next N cards  contain experimental data 
obtained  from  four  mechanical  tests  for  a  group  of  equidistantly  placed  directions 
𝜃𝑖 = 𝑖𝜋
2𝑁 , 𝑖 = 0, 1, 2, … , 𝑁.  
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FUN-I 
RUN-I 
FPS1-I 
FPS2-I 
FSH-I 
Type 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
N 
FBI 
RBI0 
LCID 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Material density 
Elastic Young’s modulus 
Poisson’s ratio 
|N|  is  order  of  Fourier  series  (i.e.,  number  of  test  groups  minus
one).  The minimum number for |N| is 2, and the maximum is 12. 
GE.0.0:  Explicit cutting-plane return mapping algorithm 
LT.0.0:  Fully implicit return mapping algorithm (more robust)
Normalized yield stress 𝜎𝑏𝑖 for equi-biaxial test. 
Strain  ratio  𝜌𝑏𝑖(0°) = 𝜀̇2(0°)/𝜀̇1(0°)  for  equi-biaxial  test  in  the 
rolling direction. 
Stress-strain curve ID.  If defined, SYS, SIP, SHS, SHL, ESH, and
E0 are ignored. 
SYS 
Static yield stress, 𝜎0.
SIP 
SHS 
SHL 
ESH 
E0 
ALPHA 
LCID2 
*MAT_CORUS_VEGTER 
DESCRIPTION
Stress increment parameter, Δ𝜎𝑚. 
Strain hardening parameter for small strain, 𝛽. 
Strain hardening parameter for larger strain, Ω. 
Exponent for strain hardening, n. 
Initial plastic strain, 𝜀0 
𝛼 distribution of hardening used in the  curve-fitting.  𝛼 = 0 pure 
kinematic  hardening  and  𝛼 = 1  provides  pure 
isotropic 
hardening. 
Curve  ID.    The  curve  defines  Young’s  modulus  scaling  factor
with  respect  to  the  plastic  strain.    By  default  it  is  assumed  that 
Young’s modulus remains constant.  Effective value is between 0
and 1. 
AOPT 
Material  axes  option  : 
EQ.0.0:  locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES,  and  then  rotated  about  the  shell  ele-
ment normal by the angle BETA. 
EQ.2.0:  globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0:  locally  orthotropic  material  axes  determined  by 
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the
element normal. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID 
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR). 
XP, YP, ZP 
Coordinates of point p for AOPT = 1. 
A1, A2, A3 
Components of vector a for AOPT = 2. 
V1, V2, V3 
Components of vector v for AOPT = 3
Figure M136-1.  Bézier interpolation curve. 
  VARIABLE   
DESCRIPTION
D1, D2, D3 
Components of vector d for AOPT = 2. 
Material angle in degrees for AOPT = 0 and 3, may be overwritten 
on the element card, see *ELEMENT_SHELL_BETA. 
Normalized yield stress 𝜎un for uniaxial test for the ith direction. 
Strain ratio (R-value) for uniaxial test for the ith direction. 
First  normalized  yield  stress  𝜎ps1  for  plain  strain  test  for  the  ith 
direction. 
Second normalized yield stress 𝜎ps2 for plain strain test for the ith 
direction. 
First  normalized  yield  stress  𝜎sh  for  pure  shear  test  for  the  ith 
direction. 
BETA 
FUN-I 
RUN-I 
FPS1-I 
FPS2-I 
FSH-I 
Remarks: 
The  Vegter  yield  locus  is  section-wise  defined  by  quadratic  Bézier  interpolation 
functions.    Each  individual  curve  uses  2  reference  points  and  a  hinge  point  in  the 
principal plane stress space, see Figure M136-1. 
The mathematical description of the Bézier interpolation is given by:
Figure M136-2.  Vegter yield surface. 
𝜎1
(
𝜎2
) = (
𝜎1
𝜎2
)
+ 2𝜇 [(
𝜎1
𝜎2
− (
𝜎1
𝜎2
)
)
] + 𝜇2 [(
𝜎1
𝜎2
+ (
𝜎1
𝜎2
)
− 2(
)
𝜎1
𝜎2
] 
)
where (𝜎1, 𝜎2)0  is  the  first  reference  point, (𝜎1, 𝜎2)1  is  the  hinge  point,  and (𝜎1, 𝜎2)2  is 
the second reference point. 𝜇 is a parameter which determines the location on the curve 
(0 ≤ 𝜇 ≤ 1).  
Four  characteristic    stress  states  are  selected  as  reference  points:  the  equi-biaxial  point 
(𝜎𝑏𝑖, 𝜎𝑏𝑖),  the  plane  strain  point  (𝜎𝑝𝑠1, 𝜎𝑝𝑠2),  the  uniaxial  point  (𝜎𝑢𝑛, 0)  and  the  pure 
shear point (𝜎𝑠ℎ, −𝜎𝑠ℎ), see Figure M136-2.  Between the 4 stress points, 3 Bézier curves 
are used to interpolate the yield locus.  Symmetry conditions are used to construct the 
complete  surface.    The  yield  locus  in  Figure  M136-2  shows  the  reference  points  of 
experiments for one specific direction.  The reference points can also be determined for 
other angles to the rolling direction (planar angle 𝜃).  E.g.  if N = 2 is chosen, normalized 
yield stresses for directions 0°, 45°, and 90° should be defined.  A Fourier series is used 
to interpolate intermediate angles between the measured points. 
The Vegter yield function with isotropic hardening (ALPHA = 1) is given as: 
𝜙 = 𝜎𝑒𝑞(𝜎1, 𝜎2, 𝜃) − 𝜎𝑦(𝜀̅𝑝)
with the equivalent stress 𝜎𝑒𝑞 obtained from the appropriate Bézier function related to 
the  current  stress  state.    The  uni-axial  yield  stress  𝜎𝑦  can  be  defined  as  stress-strain 
curve LCID or alternatively as a functional expression: 
𝜎𝑦 = 𝜎0 + Δ𝜎𝑚[𝛽(𝜀̅𝑝 + 𝜀0) + (1 − 𝑒−Ω(𝜀̅𝑝+𝜀0))
] 
In case of kinematic hardening (ALPHA < 1), the standard stress tensor is replaced by a 
relative  stress  tensor,  defined  as  the  difference  between  the  stress  tensor  and  a  back 
stress tensor. 
To  determine  the  yield  stress  or  reference  points  of  the  Vegter  yield  locus,  four 
mechanical  tests  have  to  be  performed  for  different  directions.    A  good  description  
about the material characterization procedure can be found in Vegter et al.  (2003).
*MAT_COHESIVE_MIXED_MODE 
This is Material Type 138.  This model is a simplification of *MAT_COHESIVE_GENER-
AL  restricted  to  linear  softening.    It  includes  a  bilinear  traction-separation  law  with 
quadratic mixed mode delamination criterion and a damage formulation.  This material 
model can be used only with cohesive element fomulations; see the variable ELFORM 
in *SECTION_SOLID and *SECTION_SHELL. 
6 
ET 
F 
6 
7 
8 
GIC 
GIIC 
F 
7 
F 
8 
  Card 1 
1 
2 
3 
4 
5 
Variable 
MID 
RO 
ROFLG 
INTFAIL 
EN 
Type 
A8 
  Card 2 
1 
Variable 
XMU 
Type 
F 
  VARIABLE   
MID 
F 
2 
T 
F 
F 
3 
S 
F 
F 
4 
F 
5 
UND 
UTD 
GAMMA 
F 
F 
F 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density 
ROFLG 
INTFAIL 
EN 
ET 
Flag  for  whether  density  is  specified  per  unit  area  or  volume.
ROFLG = 0  specified  density  per  unit  volume  (default),  and
ROFLG = 1  specifies  the  density  is  per  unit  area  for  controlling
the mass of cohesive elements with an initial volume of zero. 
The  number  of  integration  points  required  for  the  cohesive
element to be deleted.  If it is zero, the element will not be deleted
even if it satisfies the failure criterion.  The value of INTFAIL may
range from 1 to 4, with 1 the recommended value. 
The  stiffness  (units  of  stress / length)  normal  to  the  plane  of  the 
cohesive element. 
The stiffness (units of stress / length) in the plane of the cohesive 
element.
VARIABLE   
DESCRIPTION
GIC 
GIIC 
XMU 
T 
S 
UND 
UTD 
Energy release rate for mode I (units of stress × length) 
Energy release rate for mode II (units of stress × length) 
Exponent of the mixed mode criteria  
Peak traction (stress units) in normal direction 
LT.0.0: Load  curve  ID = (-T)  which  defines  peak  traction  in 
normal  direction  as  a  function  of  element  size.    See  re-
marks. 
Peak traction (stress units) in tangential direction 
LT.0.0: Load  curve  ID = (-S)  which  defines  peak  traction  in 
tangential  direction  as  a  function  of  element  size.    See
remarks. 
Ultimate displacement in the normal direction 
Ultimate displacement in the tangential direction 
GAMMA 
Additional exponent for Benzeggagh-Kenane law (default = 1.0) 
Remarks: 
The  ultimate  displacements 
in  the  normal  and  tangential  directions  are  the 
displacements at the time when the material has failed completely, i.e., the tractions are 
zero.    The  linear  stiffness  for  loading  followed  by  the  linear  softening  during  the 
damage provides an especially simple relationship between the energy release rates, the 
peak tractions, and the ultimate displacements: 
GIC = T ×
GIIC = S ×
UND
UTD
If  the  peak  tractions  aren’t  specified,  they  are  computed  from  the  ultimate  displace-
ments.    See  Fiolka  and  Matzenmiller  [2005]  and  Gerlach,  Fiolka  and  Matzenmiller 
[2005].  
In  this  cohesive  material  model,  the  total  mixed-mode  relative  displacement  𝛿𝑚  is 
2 , where 𝛿𝐼 = 𝛿3 is the separation in normal direction (mode I) 
defined as 𝛿𝑚 = √𝛿𝐼
2 + 𝛿𝐼𝐼
3 
2 
1 
II
traction
0δ
II
II
Fδ
Figure M138-1.  Mixed-mode traction-separation law  
and 𝛿𝐼𝐼 = √𝛿1
damage initiation displacement 𝛿0 (onset of softening) is given by 
2 is the separation in tangential direction (mode II).  The mixed-mode 
2 + 𝛿2
𝛿0 = 𝛿𝐼
0𝛿𝐼𝐼
0 √
1 + 𝛽2
0 )2 + (𝛽𝛿𝐼
(𝛿𝐼𝐼
0)2
0 = 𝑇/EN  and  𝛿𝐼𝐼
0 = 𝑆/ET  are  the  single  mode  damage  inititation  separations 
where  𝛿𝐼
and  𝛽 = 𝛿𝐼𝐼/𝛿𝐼  is  the  “mode  mixity”  .    The  ultimate  mixed-mode 
displacement 𝛿𝐹 (total failure) for the power law (XMU > 0) is: 
⎡(
⎢
⎣
and alternatively for the Benzeggagh-Kenane law [1996]  (XMU < 0): 
𝛿𝐹 =
+ (
)
)
2(1 + 𝛽2)
𝛿0
ET × 𝛽2
GIIC
EN
GIC
XMU
XMU
XMU
−   1
⎤
⎥
⎦
𝛿𝐹 =
𝛿0 ( 1
1 + 𝛽2 EN𝛾 +
1/𝛾
𝛽2
1 + 𝛽2 ET𝛾)
⎡GIC + (GIIC − GIC) (
⎢
⎣
𝛽2 × ET
EN + 𝛽2 × ET
)
|XMU|
⎤ 
⎥
⎦
A  reasonable  choice  for  the  exponent  𝛾  would  be  GAMMA = 1.0  (default)  or 
GAMMA = 2.0. 
In  this  model,  damage  of  the  interface  is  considered,  i.e.    irreversible  conditions  are 
enforced with loading/unloading paths coming from/pointing to the origin. 
Peak  tractions  𝑇  and/or 𝑆  can  be  defined  as  functions  of  characteristic  element  length 
(square root of midsurface area) via load curve.  This option is useful to get nearly the 
same  global  responses  (e.g.    load-displacement  curve)  with  coarse  meshes  when 
compared to a fine mesh solution.  In general, lower peak traction values are needed for 
coarser meshes
QMAX
GC
Displacement
Figure M138-2.  Bilinear traction-separation 
Two  error  checks  have  been  implemented  for  this  material  model  in  order  to  ensure 
proper  material  data.    Since  the  traction  versus  displacement  curve  is  fairly  simple 
(triangular  shaped),  equations  can  be  developed  to  ensure  that the  displacement,  𝐿,  at 
the peak load (QMAX), is  smaller than the  ultimate distance for failure, 𝑢.  See Figure 
M138-2 for the used notation. 
One has that 
And, 
GC =
𝑢 × QMAX 
𝐿 =
QMAX
. 
To ensure that the peak is not past the failure point, 𝑢
𝐿 must be larger than 1. 
2GC
EL
where GC is the energy release rate.  This gives  
𝑢 =
, 
=
2GC
EL × 𝐿
=
2GC
𝐸 (
QMAX
2 > 1. 
)
The error checks are then done for tension and pure shear, respectively, 
=
(2GIC)
EN( 𝑇
EN
2 > 1, 
)
=
(2GIIC)
ET ( 𝑆
ET
)
2 > 1.
*MAT_MODIFIED_FORCE_LIMITED 
This is Material Type 139.  This material for the Belytschko-Schwer resultant beam is an 
extension  of  material  29.    In  addition  to  the  original  plastic  hinge  and  collapse 
mechanisms of material 29, yield moments may be defined as a function of axial force.  
After  a  hinge  forms,  the  moment  transmitted  by  the  hinge  is  limited  by  a  moment-
plastic rotation relationship. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
DF 
F 
6 
7 
8 
AOPT 
YTFLAG 
ASOFT 
F 
F 
F 
Default 
none 
none 
none 
none 
0.0 
0.0 
0.0 
0.0 
  Card 2 
1 
Variable 
M1 
Type 
F 
Default 
none 
  Card 3 
1 
2 
M2 
F 
0 
2 
3 
M3 
F 
0 
3 
4 
M4 
F 
0 
4 
5 
M5 
F 
0 
5 
6 
M6 
F 
0 
6 
7 
M7 
F 
0 
7 
8 
M8 
F 
0 
8 
Variable 
LC1 
LC2 
LC3 
LC4 
LC5 
LC6 
LC7 
LC8 
Type 
F 
Default 
none 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LPS1 
SFS1 
LPS2 
SFS2 
YMS1 
YMS2 
Type 
Default 
F 
0 
F 
F 
F 
F 
F 
1.0 
LPS1 
1.0 
1.0E+20 YMS1 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LPT1 
SFT1 
LPT2 
SFT2 
YMT1 
YMT2 
Type 
Default 
F 
0 
F 
F 
F 
F 
F 
1.0 
LPT1 
1.0 
1.0E+20 YMT1 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LPR 
SFR 
YMR 
Type 
Default 
F 
0 
F 
F 
1.0 
1.0E+20
  Card 7 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LYS1 
SYS1 
LYS2 
SYS2 
LYT1 
SYT1 
LYT2 
SYT2 
Type 
Default 
F 
0 
F 
1.0 
F 
0 
F 
1.0 
F 
0 
F 
1.0 
F 
0 
F 
1.0
Card 8 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LYR 
SYR 
Type 
Default 
F 
0 
F 
1.0 
  Card 9 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
HMS1_1  HMS1_2  HMS1_3  HMS1_4  HMS1_5  HMS1_6  HMS1_7  HMS1_8 
Type 
Default 
F 
0 
  Card 10 
1 
F 
0 
2 
F 
0 
3 
F 
0 
4 
F 
0 
5 
F 
0 
6 
F 
0 
7 
F 
0 
8 
Variable 
LPMS1_1  LPMS1_2  LPMS1_3 LPMS1_4 LPMS1_5 LPMS1_6  LPMS1_7  LPMS1_8
Type 
Default 
F 
0 
  Card 11 
1 
F 
0 
2 
F 
0 
3 
F 
0 
4 
F 
0 
5 
F 
0 
6 
F 
0 
7 
F 
0 
8 
Variable 
HMS2_1  HMS2_2  HMS2_3  HMS2_4  HMS2_5  HMS2_6  HMS2_7  HMS2_8 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F
Card 12 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LPMS2_1  LPMS2_2  LPMS2_3 LPMS2_4 LPMS2_5 LPMS2_6  LPMS2_7  LPMS2_8
Type 
Default 
F 
0 
  Card 13 
1 
F 
0 
2 
F 
0 
3 
F 
0 
4 
F 
0 
5 
F 
0 
6 
F 
0 
7 
F 
0 
8 
Variable 
HMT1_1  HMT1_2  HMT1_3  HMT1_4  HMT1_5  HMT1_6  HMT1_7  HMT1_8 
Type 
Default 
F 
0 
  Card 14 
1 
F 
0 
2 
F 
0 
3 
F 
0 
4 
F 
0 
5 
F 
0 
6 
F 
0 
7 
F 
0 
8 
Variable 
LPMT1_1  LPMT1_2  LPMT1_3 LPMT1_4 LPMT1_5 LPMT1_6  LPMT1_7  LPMT1_8
Type 
Default 
F 
0 
  Card 15 
1 
F 
0 
2 
F 
0 
3 
F 
0 
4 
F 
0 
5 
F 
0 
6 
F 
0 
7 
F 
0 
8 
Variable 
HMT2_1  HMT2_2  HMT2_3  HMT2_4  HMT2_5  HMT2_6  HMT2_7  HMT2_8 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F
Card 16 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LPMT2_1  LPMT2_2  LPMT2_3 LPMT2_4 LPMT2_5 LPMT2_6  LPMT2_7  LPMT2_8
Type 
Default 
F 
0 
  Card 17 
1 
F 
0 
2 
F 
0 
3 
F 
0 
4 
F 
0 
5 
F 
0 
6 
F 
0 
7 
F 
0 
8 
Variable 
HMR_1 
HMR_2 
HMR_3 
HMR_4 
HMR_5 
HMR_6 
HMR_7 
HMR_8 
Type 
Default 
F 
0 
  Card 18 
1 
F 
0 
2 
F 
0 
3 
F 
0 
4 
F 
0 
5 
F 
0 
6 
F 
0 
7 
F 
0 
8 
Variable 
LPMR_1 
LPMR_2 
LPMR_3 
LPMR_4 
LPMR_5 
LPMR_6 
LPMR_7 
LPMR_8 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
DF 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s modulus 
Poisson’s ratio 
Damping  factor, see definition in  notes below.  A proper control
for the timestep has to be maintained by the user!
*MAT_MODIFIED_FORCE_LIMITED 
DESCRIPTION
AOPT 
Axial load curve option: 
EQ.0.0: axial load curves are force versus strain, 
EQ.1.0: axial load curves are force versus change in length. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
YTFLAG 
Flag to allow beam to yield in tension: 
EQ.0.0: beam does not yield in tension, 
EQ.1.0: beam can yield in tension. 
ASOFT 
M1, M2, 
…, M8 
LC1, LC2, 
…, LC8 
LPS1 
SFS1 
LPS2 
SFS2 
YMS1 
Axial  elastic  softening  factor  applied  once  hinge  has  formed.
When a hinge has formed the stiffness is reduced by this factor.  If
zero, this factor is ignored. 
Applied  end  moment  for  force  versus  (strain/change  in  length)
curve.  At least one must be defined.  A maximum of 8 moments
can be defined.  The values should be in ascending order.   
Load curve ID  defining axial force versus 
strain/change  in  length    for  the  corresponding
applied end moment.  Define the same number as end moments.
Each curve must contain the same number of points. 
Load curve ID for plastic moment versus rotation about s-axis at 
node 1.  If zero, this load curve is ignored. 
Scale factor for plastic moment versus rotation curve about s-axis 
at node 1.  Default = 1.0. 
Load curve ID for plastic moment versus rotation about s-axis at 
node 2.  Default: is same as at node 1. 
Scale factor for plastic moment versus rotation curve about s-axis 
at node 2.  Default: is same as at node 1. 
Yield  moment  about  s-axis  at  node  1  for  interaction  calculations 
(default set to 1.0E+20 to prevent interaction).
VARIABLE   
DESCRIPTION
YMS2 
LPT1 
SFT1 
LPT2 
SFT2 
YMT1 
YMT2 
LPR 
SFR 
YMR 
LYS1 
SYS1 
LYS2 
SYS2 
LYT1 
Yield  moment  about  s-axis  at  node  2  for  interaction  calculations 
(default set to YMS1). 
Load curve ID for plastic moment versus rotation about t-axis at 
node 1.  If zero, this load curve is ignored. 
Scale factor for plastic moment versus rotation curve about t-axis 
at node 1.  Default = 1.0. 
Load curve ID for plastic moment versus rotation about t-axis at 
node 2.  Default: is the same as at node 1. 
Scale factor for plastic moment versus rotation curve about t-axis 
at node 2.  Default: is the same as at node 1. 
Yield  moment  about  t-axis  at  node  1  for  interaction  calculations 
(default set to 1.0E+20 to prevent interactions) 
Yield  moment  about  t-axis  at  node  2  for  interaction  calculations 
(default set to YMT1) 
Load  curve  ID  for  plastic  torsional  moment  versus  rotation.    If
zero, this load curve is ignored. 
Scale  factor  for  plastic  torsional  moment  versus  rotation
(default = 1.0). 
Torsional yield moment for interaction calculations (default set to
1.0E+20 to prevent interaction) 
ID of curve defining yield moment as a function of axial force for
the s-axis at node 1. 
Scale factor applied to load curve LYS1. 
ID of curve defining yield moment as a function of axial force for
the s-axis at node 2. 
Scale factor applied to load curve LYS2. 
ID of curve defining yield moment as a function of axial force for
the t-axis at node 1. 
SYT1 
Scale factor applied to load curve LYT1.
LYT2 
SYT2 
LYR 
*MAT_MODIFIED_FORCE_LIMITED 
DESCRIPTION
ID of curve defining yield moment as a function of axial force for
the t-axis at node 2. 
Scale factor applied to load curve LYT2. 
ID of curve defining yield moment as a function of axial force for
the torsional axis. 
SYR 
Scale factor applied to load curve LYR. 
HMS1_n 
Hinge moment for s-axis at node 1. 
LPMS1_n 
ID  of  curve  defining  plastic  moment  as  a  function  of  plastic
rotation for the s-axis at node 1 for hinge moment HMS1_n 
HMS2_n 
Hinge moment for s-axis at node 2. 
LPMS2_n 
ID  of  curve  defining  plastic  moment  as  a  function  of  plastic
rotation for the s-axis at node 2 for hinge moment HMS2_n 
HMT1_n 
Hinge moment for t-axis at node 1. 
LPMT1_n 
ID  of  curve  defining  plastic  moment  as  a  function  of  plastic
rotation for the t-axis at node 1 for hinge moment HMT1_n 
HMT2_n 
Hinge moment for t-axis at node 2. 
LPMT2_n 
ID  of  curve  defining  plastic  moment  as  a  function  of  plastic
rotation for the t-axis at node 2 for hinge moment HMT2_n 
HMR_n 
Hinge moment for the torsional axis. 
LPMR_n 
ID  of  curve  defining  plastic  moment  as  a  function  of  plastic
rotation for the torsional axis for hinge moment HMR_n 
Remarks: 
This material model is available for the Belytschko resultant beam element only.  Plastic 
hinges form at the ends of the beam when the moment reaches the plastic moment.  The 
plastic moment versus rotation relationship is specified by the user in the form of a load 
curve  and  scale  factor.    The  points  of  the  load  curve  are  (plastic  rotation  in  radians, 
plastic  moment).    Both  quantities  should  be  positive  for  all  points,  with  the  first  point 
being  (zero,  initial  plastic  moment).    Within  this  constraint  any  form  of  characteristic 
may  be  used,  including  flat  or  falling  curves.    Different  load  curves  and  scale  factors 
may be specified at each node and about each of the local s and t axes.
Axial  collapse  occurs  when  the  compressive  axial  load  reaches  the  collapse  load.  
Collapse  load  versus  collapse  deflection  is  specified  in  the  form  of  a  load  curve.    The 
points  of  the  load  curve  are  either  (true  strain,  collapse  force)  or  (change  in  length, 
collapse force).  Both quantities should be entered as positive for all points, and will be 
interpreted as compressive.  The first point should be (zero, initial collapse load). 
The collapse load may vary with end moment as well as with deflections.  In this case 
several  load-deflection  curves  are  defined,  each  corresponding  to  a  different  end 
moment.    Each  load  curve  should  have  the  same  number  of  points  and  the  same 
deflection values.  The end moment is defined as the average of the absolute moments 
at each end of the beam and is always positive. 
Stiffness-proportional  damping  may  be  added  using  the  damping  factor  λ.    This  is 
defined as follows: 
𝜆 =
2 × 𝜉
where ξ is the damping factor at the reference frequency ω (in radians per second).  For 
example if 1% damping at 2Hz is required 
𝜆 =
2 × 0.01
2𝜋 × 2
= 0.001592 
If damping is used, a small time step may be required.  LS-DYNA does not check this so 
to avoid instability it may be necessary to control the time step via a load curve.  As a 
guide,  the  time  step  required  for  any  given  element  is  multiplied  by  0.3L⁄cλ  when 
damping is present (L = element length, c = sound speed). 
Moment Interaction: 
Plastic  hinges  can  form  due  to  the  combined  action  of  moments  about  the  three  axes.  
This facility is activated only when yield moments are defined in the material input.  A 
hinge forms when the following condition is first satisfied. 
where, 
⎜⎛ 𝑀𝑟
⎟⎞
𝑀𝑟yield⎠
⎝
+
⎜⎛ 𝑀𝑠
⎟⎞
𝑀𝑠yield⎠
⎝
+
⎜⎛ 𝑀𝑡
⎟⎞
𝑀𝑡yield⎠
⎝
≥ 1 
𝑀𝑟,  𝑀𝑠,  𝑀𝑡, = current moment 
𝑀𝑟yield,  𝑀𝑠yield,  𝑀𝑡yield = yield moment 
Note that scale factors for hinge behavior defined in the input will also be applied to the 
yield  moments:    for  example,  Msyield  in  the  above  formula  is  given  by  the  input yield 
moment about the local axis times the input scale factor for the local s axis.  For strain-
softening  characteristics,  the  yield  moment  should  generally  be  set  equal  to  the  initial 
peak of the moment-rotation load curve. 
On forming a hinge, upper limit moments are set.  These are given by  
⎜⎛𝑀𝑟,
⎝
and similar conditions hold for 𝑀𝑠𝑢𝑝𝑝𝑒𝑟and 𝑀𝑡𝑢𝑝𝑝𝑒𝑟.  Thereafter the plastic moments will 
be given by 
𝑀𝑟upper = max
⎟⎞ 
2 ⎠
𝑀𝑟yield
𝑀𝑟𝑝 = min(𝑀𝑟upper, 𝑀𝑟curve) 
where, 
𝑀𝑟p = current plastic moment 
𝑀𝑟curve = moment from load curve at the current rotation scaled by the scale factor. 
𝑀𝑠𝑝and 𝑀𝑡𝑝 satisfy similar conditions. 
The  effect  of  this  is  to  provide  an  upper  limit  to  the  moment  that can  be  generated;  it 
represents the softening effect of local buckling at a hinge site.  Thus if a member is bent 
about  is  local  s-axis  it  will  then  be  weaker  in  torsion  and  about  its  local  t-axis.    For 
moments-softening  curves,  the  effect  is  to  trim  off  the  initial  peak  (although  if  the 
curves subsequently harden, the final hardening will also be trimmed off). 
It is not possible to make the plastic moment vary with the current axial load, but it is 
possible  to  make  hinge  formation  a  function  of  axial  load  and  subsequent  plastic 
moment a function of the moment at the time the hinge formed.  This is discussed in the 
next section. 
Independent plastic hinge formation: 
In addition to the moment interaction equation, Cards 7 through 18 allow plastic hinges 
to form independently for the s-axis and t-axis at each end of the beam and also for the 
torsional  axis.    A  plastic  hinge  is  assumed  to  form  if  any  component  of  the  current 
moment  exceeds  the  yield  moment  as  defined  by  the  yield  moment  vs.    axial  force 
curves input on cards 7 and 8.  If any of the 5 curves is omitted, a hinge will not form 
for that component.  The curves can be defined for both compressive and tensile axial 
forces.  If the axial force falls outside the range of the curve, the first or last point in the 
curve will be used.  A hinge forming for one component of moment does not effect the 
other components. 
Upon  forming  a  hinge,  the  magnitude  of  that  component  of  moment  will  not  be 
permitted  to  exceed  the  current  plastic  moment..    The  current  plastic  moment  is 
obtained by interpolating between the plastic moment vs.  plastic rotation curves input
on cards 10, 12, 14, 16, or 18.  Curves may be input for up to 8 hinge moments, where 
the  hinge  moment  is  defined  as  the  yield  moment  at  the  time  that  the  hinge  formed.  
Curves must be input in order of increasing hinge moment and each curve should have 
the same plastic rotation values.  The first or last curve will be used if the hinge moment 
falls  outside  the  range  of  the  curves.    If  no  curves  are  defined,  the  plastic  moment  is 
obtain from the curves on cards 4 through 6.  The plastic moment is scaled by the scale 
factors on lines 4 to 6. 
A hinge will form if either the independent yield moment is exceeded or if the moment 
interaction equation is satisfied.  If both are true, the plastic moment will be set to the 
minimum of the interpolated value and Mrp. 
M8
M7
M6
M5
M4
M3
M2
M1M1
Strain (or change in length, see AOPT)
Figure  M139-1.   The force magnitude is limited by the  applied end  moment.
For an intermediate value of the end moment LS-DYNA interpolates between
the curves to determine the allowable force value.
*MAT_VACUUM 
This is Material Type 140.  This model is a dummy material representing a vacuum in a 
multi-material Euler/ALE model.  Instead of using ELFORM = 12 (under *SECTION_-
SOLID),  it  is  better  to  use  ELFORM = 11  with  the  void  material  defined  as  vacuum 
material instead. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
RHO 
Type 
A8 
F 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RHO 
Estimated material density.  This is used only as stability check. 
Remarks: 
1.  The vacuum density is estimated.  It should be small relative to air in the model 
(possibly at least 103 to 106 lighter than air).
*MAT_RATE_SENSITIVE_POLYMER 
This  is  Material  Type  141.    This  model,  called  the  modified  Ramaswamy-Stouffer 
model, is for the simulation of an isotropic ductile polymer with strain rate effects.  See 
references;  Stouffer  and  Dame  [1996]  and  Goldberg  and  Stouffer  [1999].    Uniaxial  test 
data is used to fit the material parameters. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
Variable 
Omega 
Type 
F 
  VARIABLE   
MID 
RO 
E 
PR 
Do 
N 
Zo 
q 
2 
RO 
F 
2 
3 
E 
F 
3 
4 
PR 
F 
4 
5 
Do 
F 
5 
6 
N 
F 
6 
7 
Zo 
F 
7 
8 
q 
F 
8 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Elastic modulus. 
Poisson's ratio 
Reference strain rate (= 1000 × max strain rate used in the test). 
Exponent  
Initial hardness of material 
. 
Omega 
Maximum internal stress.
The inelastic strain rate is defined as: 
*MAT_RATE_SENSITIVE_POLYMER 
𝐼 = 𝐷𝑜 exp
𝜀̇𝑖𝑗
⎡−0.5 (
⎢
⎣
𝑍𝑜
3𝐾2
)
𝑆𝑖𝑗 − Ω𝑖𝑗
⎟⎞ 
√𝐾2 ⎠
⎤
⎥
⎦
⎜⎛
⎝
where the 𝐾2 term is given as: 
𝐾2 = 0.5(𝑆𝑖𝑗 − Ω𝑖𝑗)(𝑆𝑖𝑗 − Ω𝑖𝑗) 
and represents the second invariant of the overstress tensor.  The elastic components of 
the  strain  are  added  to  the  inelastic  strain  to  obtain  the  total  strain.    The  following 
relationship defines the back stress variable rate: 
Ω𝑖𝑗 =
𝑞Ω𝑚𝜀̇𝑖𝑗
𝐼 − 𝑞Ω𝑖𝑗𝜀̇𝑒
𝐼 
where 𝑞 is a material constant, Ω𝑚 is a material constant that represents the maximum 
value of the internal stress, and 𝜀̇𝑒
𝐼 is the effective inelastic strain rate.
*MAT_TRANSVERSELY_ISOTROPIC_CRUSHABLE_FOAM 
This  is  Material  Type  142.    This  model  is  for  an  extruded  foam  material  that  is 
transversely isotropic, crushable, and of low density with no significant Poisson effect.  
This  material  is  used  in  energy-absorbing  structures  to  enhance  automotive  safety  in 
low  velocity  (bumper  impact)  and  medium  high  velocity  (interior  head  impact  and 
pedestrian safety) applications.  The formulation of this foam is due to Hirth, Du Bois, 
and Weimar and is documented by Du Bois [2001]. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
4 
5 
6 
E11 
E22 
E12 
E23 
F 
3 
F 
4 
F 
5 
F 
6 
7 
G 
F 
7 
8 
K 
F 
8 
Variable 
I11 
I22 
I12 
I23 
IAA 
NSYM 
ANG 
MU 
Type 
I 
  Card 3 
1 
I 
2 
I 
3 
Variable 
AOPT 
ISCL 
MACF 
Type 
F 
I 
I 
  Card 4 
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
3 
ZP 
F 
I 
4 
4 
A1 
F 
I 
5 
5 
A2 
F 
I 
6 
6 
A3 
F 
F 
7 
F 
8 
7
Variable 
1 
D1 
Type 
F 
  VARIABLE   
MID 
*MAT_TRANSVERSELY_ISOTROPIC_CRUSHABLE_FOAM 
2 
D2 
F 
3 
D3 
F 
4 
V1 
F 
5 
V2 
F 
6 
V3 
F 
7 
8 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
E11 
E22 
E12 
E23 
G 
K 
I11 
I22 
I12 
I23 
Mass density 
Elastic modulus in axial direction. 
Elastic modulus in transverse direction (E22 = E33). 
Elastic shear modulus (E12 = E31). 
Elastic shear modulus in transverse plane. 
Shear modulus. 
Bulk modulus for contact stiffness. 
Load curve for nominal axial stress versus volumetric strain. 
Load  curve  ID  for  nominal  transverse  stresses  versus  volumetric
strain (I22 = I33). 
Load  curve  ID  for  shear  stress  component  12  and  31  versus
volumetric strain (I12 = I31). 
Load  curve  ID  for  shear  stress  component  23  versus  volumetric
strain. 
IAA 
NSYM 
Load  curve  ID  (optional)  for  nominal  stress  versus  volumetric
strain for load at angle, ANG, relative to the material 𝑎-axis. 
Set  to  unity  for  a  symmetric  yield  surface  in  volumetric
compression and tension direction. 
ANG 
Angle corresponding to load curve ID, IAA.
VARIABLE   
MU 
DESCRIPTION
Damping  coefficient  for  tensor  viscosity  which  acts  in  both
tension  and  compression.    Recommended  values  vary  between
0.05 to 0.10.  If zero, tensor viscosity is not used, but bulk viscosity 
is  used  instead.    Bulk  viscosity  creates  a  pressure  as  the  element
compresses that is added to the normal stresses,  which can have
the  effect  of  creating  transverse  deformations  when  none  are
expected. 
AOPT 
Material  axes  option  : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element  nodes  as  shown  in  Figure  M2-1.    Nodes  1,  2, 
and 4 of an element are identical to the nodes used for 
the definition of a coordinate system as by *DEFINE_-
COORDINATE_NODES. 
EQ.1.0: locally orthotropic with material axes determined by a
point  in  space  and  the  global  location  of  the  element
center;  this  is  the  a-direction.    This  option  is  for  solid 
elements only. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by 
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the
element  normal.    The  plane  of  a  solid  element  is  the
midsurface  between  the  inner  surface  and  outer  sur-
face  defined  by  the  first  four  nodes  and  the  last  four 
nodes of the connectivity of the element, respectively. 
EQ.4.0: locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector  v,  and
an originating point, P, which define the centerline ax-
is.  This option is for solid elements only. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later.
ISCL 
*MAT_TRANSVERSELY_ISOTROPIC_CRUSHABLE_FOAM 
DESCRIPTION
Load  curve  ID  for  the  strain  rate  scale  factor  versus  the
volumetric  strain  rate.    The  yield  stress  is  scaled  by  the  value
specified by the load curve. 
MACF 
Material axes change flag: 
EQ.1:  No change, default, 
EQ.2:  switch material axes 𝐚 and 𝐛, 
EQ.3:  switch material axes 𝐚 and 𝐜, 
EQ.4:  switch material axes 𝐛 and 𝐜. 
XP YP ZP 
Coordinates of point 𝐩 for AOPT = 1 and 4. 
A1 A2 A3 
Components of vector 𝐚 for AOPT = 2. 
D1 D2 D3 
Components of vector 𝐝 for AOPT = 2. 
V1 V2 V3 
Define components of vector v for AOPT = 3 and 4. 
Remarks: 
This  model  behaves  in  a  more  physical  way  for  off  axis  loading  the  material  than,  for 
example,  *MAT_HONEYCOMB  which  can  exhibit  nonphysical  stiffening  for  loading 
conditions that are off axis.  The curves given for I11, I22, I12 and I23 are used to define 
a  yield  surface  of  Tsai-Wu-type  that  bounds  the  deviatoric  stress  tensor.    Hence  the 
elastic  parameters  E11,  E12,  E22  and  E23  as  well  as  G  and  K  have  to  be  defined  in  a 
consistent way.
The link ed image cannot be display ed.  The file may  hav e been mov ed, renamed, or deleted. Verify  that the link  points to the correct file and location.
  Figure M142-1.  Differences between options NSYM = 1 and NSYM = 0.
For  the  curve  definitions  volumetric  strain  𝜀𝑣 = 1 − 𝑉/𝑉0  is  used  as  the  abscissa 
parameter.  If the symmetric option (NSYM = 1) is used, a curve for the first quadrant 
has to be given only.  If NSYM = 0 is chosen, the curve definitions for I11, I22, I12 and 
I23 (and IAA) have to be in the first and second quadrant as shown in Figure M142-1.  
Tensor viscosity, which is activated by a nonzero value for MU, is generally more stable 
than  bulk  viscosity.    A  damping  coefficient  less  than  0.01  has  little  effect,  and  a  value 
greater than 0.10 may cause numerical instabilities.
*MAT_WOOD 
This is Material Type 143.  This is a transversely isotropic material and is available for 
solid elements.  The user has the option of inputting his or her own material properties 
(<BLANK>), or requesting default material properties for Southern yellow pine (PINE) 
or  Douglas  fir  (FIR).    This  model  was  developed  by  Murray  [2002]  under  a  contract 
from the FHWA. 
Available options include: 
<BLANK> 
PINE 
FIR 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
RO 
NPLOT 
ITERS 
IRATE 
GHARD 
IFAIL 
IVOL 
Type 
A8 
F 
I 
I 
I 
F 
I 
I 
Card 2 for PINE and FIR keyword options.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MOIS 
TEMP 
QUAL_T  QUAL_C 
UNITS 
IQUAL 
Type 
F 
F 
F 
F 
I 
I 
The following cards 2 through 6 are for option left blank. 
  Card 2 
Variable 
1 
EL 
Type 
F 
2 
ET 
F 
3 
4 
GLT 
GTR 
F 
F 
5 
PR 
F 
6 
7
Variable 
1 
XT 
Type 
F 
  Card 4 
1 
2 
XC 
F 
2 
3 
YT 
F 
3 
4 
YC 
F 
4 
*MAT_143 
5 
6 
7 
8 
SXY 
SYZ 
F 
5 
F 
6 
7 
8 
Variable 
GF1|| 
GF2|| 
BFIT 
DMAX|| 
GF1┴ 
GF2┴ 
DFIT 
DMAX┴ 
Type 
F 
  Card 5 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
FLPAR 
FLPARC 
POWPAR 
FLPER 
FLPERC 
POWPER 
Type 
F 
  Card 6 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
7 
8 
Variable 
NPAR 
CPAR 
NPER 
CPER 
Type 
F 
F 
F 
F 
The remaining cards all keyword options. 
  Card 7 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
AOPT 
MACF 
BETA 
Type 
F 
I
Variable 
1 
XP 
Type 
F 
  Card 9 
Variable 
1 
D1 
Type 
F 
  VARIABLE   
MID 
*MAT_WOOD 
7 
8 
7 
8 
2 
YP 
F 
2 
D2 
F 
3 
ZP 
F 
3 
D3 
F 
4 
A1 
F 
4 
V1 
F 
5 
A2 
F 
5 
V2 
F 
6 
A3 
F 
6 
V3 
F 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density 
NPLOT 
Controls  what  is  written  as  component  7  to  the  d3plot  database.
LS-PrePost  always  blindly  labels  this  component  as  effective
plastic strain.: 
EQ.1: Parallel damage (default). 
EQ.2: Perpendicular damage. 
ITERS 
Number  of  plasticity  algorithm  iterations.    The  default  is  one
iteration. 
IRATE 
Rate effects option: 
EQ.0: Rate effects model turned off (default). 
EQ.1: Rate effects model turned on. 
GHARD 
Perfect  plasticity  override.    Values  greater  than  or  equal  to  zero
are  allowed.    Positive  values  model  late  time  hardening  in
compression  (an  increase  in  strength  with  increasing  strain).    A
zero value models perfect plasticity (no increase in strength with 
increasing strain).  The default is zero. 
IFAIL 
Erosion perpendicular to the grain. 
EQ.0: No (default).
EQ.1: Yes (not recommended except for debugging). 
IVOL 
Flag  to  invoke  erosion  based  on  negative  volume  or  strain
increments greater than 0.01. 
EQ.0: No, do not apply erosion criteria. 
EQ.1: Yes, apply erosion criteria. 
MOIS 
TEMP 
QUAL_T 
Percent moisture content.  If left blank, moisture content defaults 
to saturated at 30%. 
Temperature  in  ˚C.    If  left  blank,  temperature  defaults  to  room
temperature at 20 ˚C 
Quality  factor  options.    These  quality  factors  reduce  the  clear
wood  tension,  shear,  and  compression  strengths  as  a  function  of
grade. 
EQ.0:  Grade 1, 1D, 2, 2D. 
Predefined strength reduction factors are: 
Pine:  QUAL_T = 0.47 in tension/shear. 
  QUAL_C = 0.63 in compression. 
Fir: 
QUAL_T = 0.40 in tension/shear 
  QUAL_C = 0.73 in compression. 
EQ.-1:  DS-65 or SEl STR (pine and fir). 
Predefined strength reduction factors are: 
  QUAL_T = 0.80 in tension/shear. 
  QUAL_C = 0.93 in compression. 
EQ.-2:  Clear wood. 
No strength reduction factors are applied: 
  QUAL_T = 1.0. 
  QUAL_C = 1.0. 
GT.0:  User defined quality factor in tension.  Values between
0  and  1  are  expected.    Values  greater  than  one  are  al-
lowed, but may not be realistic. 
QUAL_C 
User  defined  quality  factor  in  compression.    This  input  value  is
used if Qual_T > 0.  Values between 0 and 1 are expected.  Values 
greater  than  one  are  allowed,  but  may  not  be  realistic.    If  left
blank, a default value of Qual_C = Qual_T is used.
UNITS 
Units options: 
EQ.0: GPa, mm, msec, Kg/mm3, kN. 
EQ.1: MPa, mm, msec, g/mm3, Nt. 
EQ.2: MPa, mm, sec, Mg/mm3, Nt. 
EQ.3: Psi, inch, sec, lb-s2/inch4, lb 
IQUAL 
Apply quality factors perpendicular to the grain: 
EQ.0: Yes (default). 
EQ.1: No. 
Parallel normal modulus 
Perpendicular normal modulus. 
Parallel shear modulus (GLT = GLR). 
Perpendicular shear modulus. 
Parallel major Poisson's ratio. 
Parallel tensile strength. 
Parallel compressive strength. 
Perpendicular tensile strength. 
Perpendicular compressive strength. 
Parallel shear strength. 
Perpendicular shear strength. 
EL 
ET 
GLT 
GTR 
PR 
XT 
XC 
YT 
YC 
SXY 
SYZ 
GF1|| 
GF2|| 
Parallel fracture energy in tension. 
Parallel fracture energy in shear. 
BFIT 
Parallel softening parameter. 
DMAX|| 
Parallel maximum damage. 
Perpendicular fracture energy in tension. 
Perpendicular fracture energy in shear. 
GF1┴ 
GF2┴
DFIT 
Perpendicular softening parameter. 
DMAX┴ 
Perpendicular maximum damage. 
FLPAR 
Parallel fluidity parameter for tension and shear. 
FLPARC 
Parallel fluidity parameter for compression. 
POWPAR 
Parallel power. 
FLPER 
Perpendicular fluidity parameter for tension and shear. 
FLPERC 
Perpendicular fluidity parameter for compression. 
POWPER 
Perpendicular power. 
NPAR 
Parallel hardening initiation. 
CPAR 
NPER 
CPER 
AOPT 
Parallel hardening rate 
Perpendicular hardening initiation. 
Perpendicular hardening rate. 
Material axes option : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element  nodes  as  shown  in  Figure  M2-1.    Nodes  1,  2, 
and 4 of an element are identical to the nodes used for
the definition of a coordinate system as by *DEFINE_-
COORDINATE_NODES. 
EQ.1.0: locally orthotropic with material axes determined by a
point  in  space  and  the  global  location  of  the  element 
center;  this  is  the  a-direction.    This  option  is  for  solid 
elements only. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by 
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the
element  normal.    The  plane  of  a  solid  element  is  the
midsurface between the inner surface and outer surface 
defined by the first four nodes and the last four nodes
of the connectivity of the element, respectively. 
EQ.4.0: locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector  v,  and 
an originating point, P, which define the centerline ax-
is.  This option is for solid elements only. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
MACF 
Material axes change flag: 
EQ.1: No change, default, 
EQ.2: switch material axes a and b, 
EQ.3: switch material axes a and c, 
EQ.4: switch material axes b and c. 
BETA 
Material  angle  in  degrees  for  AOPT = 3,  may  be  overridden  on 
the element card, see *ELEMENT_SOLID_ORTHO. 
XP YP ZP 
Coordinates of point p for AOPT = 1 and 4. 
A1 A2 A3 
Components of vector a for AOPT = 2. 
D1 D2 D3 
Components of vector d for AOPT = 2. 
V1 V2 V3 
Define components of vector v for AOPT = 3 and 4. 
Remarks: 
Material  property  data  is  for  clear  wood  (small  samples  without  defects  like  knots), 
whereas  real  structures  are  composed  of  graded  wood.    Clear  wood  is  stronger  than 
graded wood.  Quality factors (strength reduction factors) are applied to the clear wood 
strengths to account for reductions in strength as a function of grade.  One quality factor 
(QUAL_T)  is  applied  to  the  tensile  and  shear  strengths.    A  second  quality  factor 
(QUAL_C)  is  applied  to  the  compressive  strengths.    As  a  option,  predefined  quality 
factors are provided based on correlations between LS-DYNA calculations and test data 
for pine and fir posts impacted by bogie vehicles.  By default, quality factors are applied 
to  both  the  parallel  and  perpendicular  to  the  grain  strengths.    An  option  is  available 
(IQUAL) to eliminate application perpendicular to the grain.
*MAT_PITZER_CRUSHABLE_FOAM 
This is Material Type 144.  This model is for the simulation of isotropic crushable forms 
with strain rate effects.  Uniaxial and triaxial test data have to be used.  For the elastic 
response, the Poisson ratio is set to zero. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
K 
F 
3 
Variable 
LCPY 
LCUYS 
LCSR 
Type 
I 
I 
I 
6 
TY 
F 
6 
7 
8 
SRTV 
F 
7 
8 
4 
G 
F 
4 
VC 
F 
5 
PR 
F 
5 
DFLG 
F 
DESCRIPTION
  VARIABLE   
MID 
RO 
K 
G 
PR 
TY 
SRTV 
LCPY 
LCUYS 
LCSR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Bulk modulus. 
Shear modulus 
Poisson's ratio 
Tension yield. 
Young’s modulus (E) 
Load  curve  ID  giving  pressure  versus  volumetric  strain,  see
Figure M75-1. 
Load curve ID giving uniaxial stress versus volumetric strain, see
Figure M75-1. 
Load  curve  ID  giving  strain  rate  scale  factor  versus  volumetric
strain rate.
*MAT_PITZER_CRUSHABLE_FOAM 
DESCRIPTION
VC 
Viscous damping coefficient (.05 < recommended value < .50). 
DFLG 
Density flag: 
EQ.0.0: use initial density 
EQ.1.0: use  current  density  (larger  step  size  with  less  mass
scaling). 
Remarks: 
The logarithmic volumetric strain is defined in terms of the relative volume, 𝑉, as: 
𝛾 = −ln(𝑉) 
In defining the curves the stress and strain pairs should be positive values starting with 
a volumetric strain value of zero.
*MAT_SCHWER_MURRAY_CAP_MODEL 
This is Material Type 145.  *MAT_145 is a Continuous Surface Cap Model and is a three 
invariant  extension  of  *MAT_GEOLOGIC_CAP_MODEL  (*MAT_025)  that  includes 
viscoplasticity  for  rate  effects  and  damage  mechanics  to  model  strain  softening.    The 
primary  references  for  the  model  are  Schwer  and  Murray  [1994],  Schwer  [1994],  and 
Murray and Lewis [1994].   *MAT_145 was developed for geomaterials including soils, 
concrete,  and  rocks.    It  is  recommended  that  an  updated  version  of  a  Continuous 
Surface Cap Model, *MAT_CSCM (*MAT_159), be used rather than *MAT_SCHWER_-
MURRAY_CAP_MODEL (*MAT_145). 
Warning: no default input parameter values are assumed, but recommendations for the 
more obscure parameters are provided in the descriptions that follow. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
RO 
SHEAR 
BULK 
GRUN 
SHOCK 
PORE 
Type 
A8 
  Card 2 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
8 
Variable 
ALPHA 
THETA 
GAMMA 
BETA 
EFIT 
FFIT 
ALPHAN 
CALPHA 
Type 
F 
F 
  Card 3 
1 
Variable 
RO 
Type 
F 
  Card 4 
Variable 
Type 
1 
W 
F 
2 
XO 
F 
2 
D1 
F 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
IROCK 
SECP 
AFIT 
BFIT 
RDAMO 
F 
3 
D2 
F 
F 
4 
F 
5 
F 
6 
F 
7 
NPLOT 
EPSMAX 
CFIT 
DFIT 
TFAIL 
F 
F 
F 
F 
F 
F 
8
Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FAILFL 
DBETA 
DDELTA 
VPTAU 
Type 
F 
  Card 6 
1 
F 
2 
F 
3 
F 
4 
5 
6 
7 
8 
Variable 
ALPHA1 
THETA1  GAMMA1
BETA1 
ALPHA2 
THETA2  GAMMA2 
BETA2 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density 
SHEAR 
Shear modulus, G 
BULK 
Bulk modulus, K 
GRUN 
Gruneisen ratio (typically  = 0), Γ 
SHOCK 
Shock velocity parameter (typically 0), Sl 
PORE 
Flag for pore collapse 
EQ.0.0:  for Pore collapse 
EQ.1.0:  for Constant bulk modulus (typical) 
ALPHA 
Shear failure parameter, 𝛼 
THETA 
Shear failure parameter, 𝜃 
GAMMA 
Shear failure parameter, 𝛾 
BETA 
Shear failure parameter, 𝛽 
√𝐽′2 = 𝐹𝑒(𝐽1) = 𝛼 − 𝛾exp(−𝛽𝐽1) + 𝜃𝐽1 
EFIT 
Dilitation damage mechanics parameter (no damage = 1)
VARIABLE   
DESCRIPTION
FFIT 
Dilitation damage mechanics parameter (no damage = 0) 
ALPHAN 
Kinematic strain hardening parameter, 𝑁𝛼 
CALPHAN 
Kinematic strain hardening parameter, 𝑐𝛼 
R0 
X0 
Initial cap surface ellipticity, R 
Initial cap surface 𝐽1 (mean stress) axis intercept, 𝑋(𝜅0) 
IROCK 
EQ.0:  soils (cap can contract) 
EQ.1:  rock/concrete 
Shear enhanced compaction 
Ductile damage mechanics parameter (=1 no damage) 
Ductile damage mechanics parameter (=0 no damage) 
SECP 
AFIT 
BFIT 
RDAM0 
Ductile damage mechanics parameter 
W 
D1 
D2 
Plastic Volume Strain parameter, W 
Plastic Volume Strain parameter, D1 
Plastic Volume Strain parameter, D2 
NPLOT 
EPSMAX 
CFIT 
DFIT 
𝑃 = 𝑊{1 − exp{−𝐷1[𝑋(𝜅) − 𝑋(𝜅0)] − 𝐷2[(𝑋(𝜅) − 𝑋(𝜅0)]2}} 
𝜀𝑉
History variable post-processed as effective plastic strain 
 
Maximum permitted strain increment (default = 0) 
Δ𝜀max = 0.05(𝛼 − 𝑁𝛼 − 𝛾)min( 1
9𝐾) (calculated default) 
𝐺, 𝑅
Brittle damage mechanics parameter (=1 no damage) 
Brittle damage mechanics parameter (=0 no damage) 
TFAIL 
Tensile failure stress
FAILFL 
*MAT_SCHWER_MURRAY_CAP_MODEL 
DESCRIPTION
Flag controlling element deletion and effect of damage on stress 
: 
EQ.1:  𝜎𝑖𝑗  reduces  with  increasing  damage;  element  is  deleted
when fully damaged (default) 
EQ.-1:  𝜎𝑖𝑗  reduces  with  increasing  damage;  element  is  not
deleted 
EQ.2:  𝑆𝑖𝑗  reduces  with  increasing  damage;  element  is  deleted
when fully damaged 
EQ.-2:  𝑆𝑖𝑗  reduces  with  increasing  damage;  element  is  not
deleted 
DBETA 
Rounded vertices parameter, Δ𝛽0 
DDELTA 
Rounded vertices parameter, 𝛿 
VPTAU 
Viscoplasticity relaxation time parameter, 𝜏 
ALPHA1 
Torsion scaling parameter, 𝛼1 
𝛼1 < 0 → |𝛼1| = Friction Angle (degrees) 
THETA1 
Torsion scaling parameter, 𝜃1 
GAMMA1 
Torsion scaling parameter, 𝛾1 
BETA1 
Torsion scaling parameter, 𝛽1 
𝑄1 = 𝛼1 − 𝛾1exp(−𝛽1𝐽1) + 𝜃1𝐽1𝜃2 
ALPHA2 
Tri-axial extension scaling parameter, 𝛼2 
THETA2 
Tri-axial extension scaling parameter,𝜃2  
GAMMA2 
Tri-axial extension scaling parameter, 𝛾2 
BETA2 
Tri-axial extension scaling parameter, 𝛽2 
𝑄2 = 𝛼2 − 𝛾2exp(−𝛽2𝐽1) + 𝜃2𝐽1 
Remarks: 
1.  FAILFL  controls  whether  the  damage  accumulation  applies  to  either  the  total 
stress  tensor𝜎𝑖𝑗or  the  deviatoric  stress  tensor𝑆𝑖𝑗.    When  FAILFL = 2,  damage 
does not diminish the ability of the material to support hydrostatic stress.
2.  FAILFL  also  serves  as  a  flag  to  control  element  deletion.    Fully  damaged 
elements are deleted only if FAILFL is a positive value.  When MAT_145 is used 
with  the  ALE  or  EFG  solvers,  failed  elements  should  not  be  eroded  and  so  a 
negative value of FAILFL should be used. 
Output History Variables: 
All the output parameters listed in Table M145-1 is available for post-processing using 
LS-PrePost and its displayed list of History Variables.  The LS-DYNA input parameter 
NEIPH  should  be  set  to  26;  see  for  example  the  keyword  input  for  *DATABASE_EX-
TENT_BINARY. 
PLOT 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
11 
12 
13 
14 
15 
16 
17 
18 
19 
20 
21 
22 
23 
24 
25 
26 
Function
𝑋(𝜅) 
𝐿(𝜅) 
𝑅 
𝑅̃  
𝑝 
𝜀𝜈
𝐺𝛼 
𝛼 
𝐽2
𝛽 
d 
Description
𝐽1 intercept of cap surface 
𝐽1value at cap-shear surface intercept 
Cap surface ellipticity 
Rubin function 
Plastic volume strain 
Yield Flag ( = 0 elastic) 
Number of strain sub-increments 
Kinematic hardening parameter 
Kinematic hardening back stress 
Effective strain rate 
Ductile damage 
Ductile damage threshold 
Strain energy 
Brittle damage 
Brittle damage threshold 
Brittle energy norm 
𝐽1 (w/o visco-damage/plastic) 
𝐽′2 (w/o visco-damage/plastic) 
𝐽′3 (w/o visco-damage/plastic) 
𝐽 ̂3(w/o visco-damage/plastic) 
Lode Angle 
Maximum damage parameter 
future variable 
future variable 
future variable 
future variable 
Table M145-1.  Output variables for post-processing using NPLOT parameter.
*MAT_SCHWER_MURRAY_CAP_MODEL 
Gran  and  Senseny  [1996]  report  the  axial  stress  versus  strain  response  for  twelve 
unconfined compression tests of concrete, used in scale-model reinforced-concrete wall 
tests.    The  Schwer  &  Murray  Cap  Model  parameters  provided  below  were  used,  see 
Schwer [2001], to model the unconfined compression test stress-strain response for the 
nominal 40 MPa strength concrete reported by Gran and Senseny.  The basic units for 
the  provided  parameters  are  length  in  millimeters  (mm),  time  in  milliseconds  (msec), 
and  mass  in  grams  (g).    This  base  unit  set  yields  units  of  force  in  Newtons  (N)  and 
pressure in Mega-Pascals (MPa). 
Example MAT_SCHWER_MURRAY_CAP_MODEL deck 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
RO 
SHEAR 
BULK 
GRUN 
SHOCK 
PORE 
Value 
A8 
2.3E-3  1.048E4 1.168E4
0.0 
0.0 
1. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ALPHA 
THETA 
GAMMA 
BETA 
EFIT 
FFIT 
ALPHAN 
CALPHA 
Value 
190.0 
0.0 
184.2 
2.5E-3 
0.999 
0.7 
2.5 
2.5E3 
  Card 3 
Variable 
1 
R0 
2 
X0 
3 
4 
5 
6 
7 
8 
IROCK 
SECP 
AFIT 
BFIT 
RDAM0 
Value 
5.0 
100.0 
1.0 
0.0 
0.999 
0.3 
0.94 
  Card 4 
Variable 
1 
W 
2 
D1 
3 
D2 
4 
5 
6 
7 
8 
NPLOT 
EPSMAX 
CFIT 
DFIT 
TFAIL 
Value 
5.0E-2  2.5E-4  3.5E-7 
23.0 
0.0 
1.0 
300.0 
7.0
Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FAILFG 
DBETA 
DDELTA 
VPTAU 
Value 
1.0 
0.0 
0.0 
0.0 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ALPHA1 
THETA1  GAMMA1
BETA1 
ALPHA2 
THETA2  GAMMA2 
BETA2 
Value 
0.747 
3.3E-4 
0.17 
5.0E-2 
0.66 
4.0E-4 
0.16 
5.0E-2 
User Input Parameters and System of Units 
Consider the following basic units: 
Length:  𝐿 (e.g.  millimeters - mm ) 
Mass:  M (e.g.  grams - g ) 
Time:  T (e.g.  milliseconds - ms ) 
The  following  consistent  unit  systems  can  then  be  derived  using  Newton's  Law,  i.e. 
𝐹 = 𝑀𝑎. 
Force:  𝐹 = 𝑀𝐿/𝑇2 [ g-mm/ms 2= Kg-m/s 2= Newton - N ] 
Stress:  𝜎 = 𝐹/L2 [ N/mm 2 = 10 6N/m 2 = 10 6 Pascals = MPa ] 
Density: ρ = M/L3 [ g/mm 3 = 10 6 Kg/m 3 ] 
User Inputs and Units 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
RO 
SHEAR 
BULK 
GRUN 
SHOCK 
PORE 
Units 
I 
Density 
M/L3 
Stress:
F/L2 
Stress:
F/L2
Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ALPHA 
THETA 
GAMMA 
BETA 
EFIT 
FFIT 
ALPHAN 
CALPHA 
Units 
Stress: 
F/L2 
Stress:
F/L2 
Stress-1:
L2/F 
Stress-½: 
L/F½ 
Stress: 
F/L2 
Stress:
F/L2 
  Card 3 
Variable 
1 
R0 
2 
X0 
3 
4 
5 
6 
7 
8 
IROCK 
SECP 
AFIT 
BFIT 
RDAM0 
Units 
Stress: 
F/L2 
Stress-½: 
L/F½ 
Stress½: 
F½/L 
  Card 4 
Variable 
1 
W 
2 
D1 
3 
D2 
4 
5 
6 
7 
8 
NPLOT  MAXEPS 
CFIT 
DFIT 
TFAIL 
Units 
Stress-1: 
L2/F 
Stress-2:
L4/F2 
Stress-½: 
L/F½ 
Stress:
F/L2 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FAILFG 
DBETA 
DDELTA 
VPTAU 
Units 
Angle 
degrees 
Time T 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ALPHA1 
THETA1  GAMMA1
BETA1 
ALPHA2 
THETA2  GAMMA2 
BETA2 
Units 
Stress: 
F/L2 
Stress:
F/L2 
Stress-1:
L2/F 
Stress:
F/L2 
Stress: 
F/L2 
Stress-1:
L2/F
*MAT_1DOF_GENERALIZED_SPRING 
This  is  Material  Type  146.    This  is  a  linear  spring  or  damper  that  allows  different 
degrees-of-freedom at two nodes to be coupled. 
3 
K 
F 
3 
4 
C 
F 
4 
5 
6 
7 
8 
SCLN1 
SCLN2 
DOFN1 
DOFN2 
F 
5 
F 
6 
I 
7 
I 
8 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
Variable 
CID1 
CID2 
Type 
I 
I 
  VARIABLE   
DESCRIPTION
MID 
RO 
K 
C 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density, see also volume in *SECTION_BEAM definition. 
Spring stiffness. 
Damping constant. 
SCLN1 
Scale factor on force at node 1.  Default = 1.0. 
SCLN2 
Scale factor on force at node 2.  Default = 1.0. 
DOFN1 
DOFN2 
Active  degree-of-freedom  at  node  1,  a  number  between  1  to  6
where  1  is  x-translation  and  4  is  x-rotation.    If  this  parameter  is 
defined in the SECTION_BEAM definition or on the ELEMENT_-
BEAM_SCALAR card, then the value here, if defined, is ignored. 
Active degree-of-freedom at node 2, a number between 1 to 6.  If
this parameter is defined in the SECTION_BEAM definition or on 
the  ELEMENT_BEAM_SCALAR  card,  then  the  value  here,  if 
defined, is ignored.
CID1 
*MAT_1DOF_GENERALIZED_SPRING 
DESCRIPTION
Local coordinate system at node 1.  This coordinate system can be
overwritten  by  a  local  system  specified  on  the  *ELEMENT_-
BEAM_SCALAR  or  *SECTION_BEAM  keyword  input.    If  no 
coordinate system is specified, the global system is used. 
CID2 
Local coordinate system at node 2.  If CID2 = 0,  CID2 = CID1.
*MAT_147 
This is Material Type 147.  This is an isotropic material with damage and is available for 
solid  elements.    The  model  has  a  modified  Mohr-Coulomb  surface  to  determine  the 
pressure  dependent  peak  shear  strength.    It  was  developed  for  applications  involving 
roadbase  soils  by  Lewis  [1999]  for  the  FHWA,  who  extended  the  work  of  Abbo  and 
Sloan [1995] to include excess pore water effects. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
RO 
NPLOT 
SPGRAV  RHOWAT 
VN 
GAMMAR 
INTRMX 
Type 
A8 
F 
Default 
none 
none 
  Card 2 
Variable 
Type 
1 
K 
F 
2 
G 
F 
I 
1 
3 
F 
F 
F 
F 
none 
1.0 
0.0 
0.0 
4 
5 
6 
7 
PHIMAX 
AHYP 
COH 
ECCEN 
AN 
I 
1 
8 
ET 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MCONT 
PWD1 
PWKSK 
PWD2 
PHIRES 
DINT 
VDFM 
DAMLEV 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
0.0 
none 
none 
none
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EPSMAX 
Type 
F 
Default 
none 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density 
NPLOT 
Controls  what  is  written  as  component  7  to  the  d3plot  database.
LS-PrePost  always  blindly  labels  this  component  as  effective
plastic strain. 
EQ.1: Effective Strain 
EQ.2: Damage Criterion Threshold 
EQ.3: Damage (diso) 
EQ.4: Current Damage Criterion 
EQ.5: Pore Water Pressure 
EQ.6: Current Friction Angle (phi) 
SPGRAV 
Specific Gravity of Soil used to get porosity. 
RHOWATt 
Density  of  water  in  model  units  -  used  to  determine  air  void 
strain (saturation) 
VN 
Viscoplasticity parameter (strain-rate enhanced strength) 
GAMMAr 
Viscoplasticity parameter (strain-rate enhanced strength) 
ITERMAXx 
Maximum number of plasticity iterations (default 1) 
K 
G 
Bulk Modulus (non-zero) 
Shear modulus (non-zero) 
PHIMAX 
Peak Shear Strength Angle (friction angle) (radians)
VARIABLE   
DESCRIPTION
AHYP 
Coefficient A for modified Drucker-Prager Surface 
COH 
Cohesion ñ Shear Strength at zero confinement (overburden) 
ECCEN 
Eccentricity parameter for third invariant effects 
AN 
ET 
MCONT 
Strain hardening percent of phi max where non-linear effects start
Strain Hardening Amount of non-linear effects 
Moisture  Content  of  Soil  (Determines  amount  of  air  voids)  (0.0 -
1.00) 
PWD1 
Parameter for pore water effects on bulk modulus 
PWKSK 
PWD2 
PHIRES 
Skeleton  bulk  modulus-  Pore  water  parameter  ñ  set  to  zero  to 
eliminate effects 
Parameter  for  pore  water  effects  on  the  effective  pressure
(confinement) 
The  minimum  internal  friction  angle,  radians  (residual  shear 
strength) 
DINT 
Volumetric Strain at Initial damage threshold, EMBED Equation.3 
VDFM 
Void formation energy (like fracture energy) 
DAMLEV 
Level of damage that will cause element deletion (0.0 - 1.00)   
EPSMAX 
Maximum principle failure strain
*MAT_FHWA_SOIL_NEBRASKA 
This  is  an  option  to  use  the  default  properties  determined  for  soils  used  at  the 
University  of  Nebraska  (Lincoln).    The  default  units  used  for  this  material  are 
millimeter,  millisecond,  and  kilograms.    If  different  units  are  desired,  the  conversion 
factors must be input. 
This is Material Type 147.  This is an isotropic material with damage and is available for 
solid  elements.    The  model  has  a  modified  Mohr-Coulomb  surface  to  determine  the 
pressure  dependent  peak  shear  strength.    It  was  developed  for  applications  involving 
road base soils. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
FCTIM 
FCTMAS 
FCTLEN 
Type 
A8 
F 
Default 
none 
none 
I 
1 
F 
F 
F 
F 
none 
1.0 
0.0 
0.0 
I 
1 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
FCTIM 
Factor to multiply milliseconds by to get desired time units 
FCTMAS 
Factor to multiply kilograms by to get desired mass units 
FCTLEN 
Factor to multiply millimeters by to get desired length units 
Remarks: 
1.  As an example, if time units of seconds are desired, then FCTIM = 0.001
*MAT_148 
This  is  Material  Type  148.    This  model  is  for  the  simulation  of  thermally  equilibrated 
ideal  gas  mixtures.    This  only  works  with  the  multi-material  ALE  formulation 
(ELFORM = 11  in  *SECTION_SOLID).    This  keyword  needs  to  be  used  together  with 
*INITIAL_GAS_MIXTURE  for  the  initialization  of  gas  densities  and  temperatures.  
When  applied  in  the  context  of  ALE  airbag  modeling,  the  injection  of  inflator  gas  is 
done  with  a  *SECTION_POINT_SOURCE_MIXTURE  command  which  controls  the 
injection  process.    This  material  model  type  also  has  its  name  start  with  *MAT_ALE_.  
For  example,  an  identical  material  model  to  this  is  *MAT_ALE_GAS_MIXTURE  (or 
also, *MAT_ALE_02). 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
IADIAB 
RUNIV 
Type 
A8 
Default 
none 
Remark 
I 
0 
5 
F 
0.0 
1 
Card 2 for Per mass Calculation.  Method (A) RUNIV = blank or 0.0. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  CVmass1  CVmass2  CVmass3 CVmass4 CVmass5 CVmass6  CVmass7  CVmass8
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none
Card 3 for Per mass Calculation.  Method (A) RUNIV = blank or 0.0. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  CPmass1  CPmass 2  CPmass 3 CPmass 4 CPmass 5 CPmass6  CPmass 7  CPmass 8
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Card 2 for Per Mole Calculation.  Method (B) RUNIV is nonzero. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MOLWT1  MOLWT2  MOLWT3 MOLWT4 MOLWT5 MOLWT6  MOLWT7  MOLWT8
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Remark 
2 
Card 3 for Per Mole Calculation.  Method (B) RUNIV is nonzero. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CPmole1  CPmole2  CPmole3  CPmole4  CPmole5  CPmole6  CPmole7  CPmole8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Remark
Card 4 for Per Mole Calculation.  Method (B) RUNIV is nonzero. 
  Card 4 
Variable 
1 
B1 
Type 
F 
2 
B2 
F 
3 
B3 
F 
4 
B4 
F 
5 
B5 
F 
6 
B6 
F 
7 
B7 
F 
8 
B8 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Remark 
2 
Card 5 for Per Mole Calculation.  Method (B) RUNIV is nonzero. 
  Card 5 
Variable 
1 
C1 
Type 
F 
2 
C2 
F 
3 
C3 
F 
4 
C4 
F 
5 
C5 
F 
6 
C6 
F 
7 
C7 
F 
8 
C8 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Remark 
2 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
IADIAB 
This  flag  (default = 0)  is  used  to  turn  ON/OFF  adiabatic 
compression logics for an ideal gas (remark 5). 
EQ.0: OFF (default) 
EQ.1: ON 
RUNIV 
Universal gas constant in per-mole unit (8.31447 J/(mole*K)). 
CVmass1 -
CVmass8 
If  RUNIV  is  BLANK  or  zero  (method  A):  Heat  capacity  at
constant volume for up to eight different gases in per-mass unit.
𝐶𝑝(𝑇) 
CPmole
kg K
mole K
mole K2 
𝐶 
mole K3 
Figure M148-1.  Standard SI units. 
  VARIABLE   
DESCRIPTION
If  RUNIV  is  BLANK  or  zero  (method  A):  Heat  capacity  at 
constant pressure for up to eight different gases in per-mass unit.
If RUNIV is nonzero (method B):  Molecular weight of each ideal
gas in the mixture (mass-unit/mole). 
If  RUNIV  is  nonzero  (method  B):  Heat  capacity  at  constant 
pressure  for  up  to  eight  different  gases  in  per-mole  unit.    These 
are  nominal  heat  capacity  values  typically  at  STP.    These  are
denoted by the variable “A” in the equation in remark 2. 
If  RUNIV  is  nonzero  (method  B):  First  order  coefficient  for  a 
temperature dependent heat capacity at constant pressure for up
to eight different gases.  These are denoted by the variable “B” in
the equation in remark 2. 
If  RUNIV  is  nonzero  (method  B):  Second  order  coefficient  for  a
temperature dependent heat capacity at constant pressure for up
to eight different gases.  These are denoted by the variable “C” in
the equation in remark 2. 
CPmass1 -
CPmass8 
MOLWT1 -
MOLWT8 
CPmole1 - 
CPmole8 
B1 - B8 
C1 - C8 
Remarks: 
1.  There are 2 methods of defining the gas properties for the mixture.  If RUNIV is 
BLANK  or  ZERO  →  Method  (A)  is  used  to  define  constant  heat  capacities 
where  per-mass  unit  values  of  Cv  and  Cp  are  input.    Only  cards  2  and  3  are 
required for this method.  Method (B) is used to define constant or temperature 
dependent heat capacities where per-mole unit values of Cp are input.  Cards 2 - 
5 are required for this method. 
2.  The per-mass-unit, temperature-dependent, constant-pressure heat capacity is 
𝐶𝑝(𝑇) =
[CPmole + 𝐵 × 𝑇 + 𝐶 × 𝑇2]
MOLWT
See table M148-1.
3.  The initial temperature and the density of the gas species present in a mesh or 
part at time zero is specified by the keyword *INITIAL_GAS_MIXTURE. 
4.  The ideal gas mixture is assumed to be thermal equilibrium, that is, all species 
are at the same temperature (T).  The gases in the mixture are also assumed to 
follow Dalton’s Partial Pressure Law, 𝑃 = ∑ 𝑃𝑖
.  The partial pressure of each 
𝑅univ
𝑀𝑊 .  The individual gas species temper-
gas is then 𝑃𝑖 = 𝜌𝑖𝑅gas𝑖
ature equals the mixture temperature.  The temperature is computed from the 
internal energy where the mixture internal energy per unit volume is used, 
𝑇 where 𝑅gas𝑖
ngas
=
ngas
𝑒𝑉 = ∑ 𝜌𝑖𝐶𝑉𝑖
ngas
𝑇𝑖 = ∑ 𝜌𝑖𝐶𝑉𝑖
𝑇 
𝑇 = 𝑇𝑖 =
𝑒𝑉
ngas
∑ 𝜌𝑖𝐶𝑉𝑖
In  general,  the  advection  step  conserves  momentum  and  internal  energy,  but 
not  kinetic  energy.    This  can  result  in  energy  lost  in  the  system  and  lead  to  a 
pressure  drop.    In  *MAT_GAS_MIXTURE  the  dissipated  kinetic  energy  is  au-
tomatically converted into heat (internal energy).  Thus in effect the total energy 
is  conserved  instead  of  conserving  just  the  internal  energy.    This  numerical 
scheme has been shown to improve accuracy in some cases.  However, the user 
should always be vigilant and check the physics of the problem closely. 
5.  As an example  consider an airbag surrounded by ambient air.  As the inflator 
gas flows into the bag, the ALE elements cut by the airbag fabric shell elements 
will contain some inflator gas inside and some ambient air outside.  The multi-
material element treatment is not perfect.  Consequently the temperature of the 
outside  air  may  be  made  artificially  high  after  the  multi-material  element 
treatment.    To  prevent  the outside  ambient  air  from  getting  artificially  high  T, 
set IDIAB = 1 for the ambient air outside.  Simple adiabatic compression equa-
tion is then assumed for the outside air.  The use of this flag may be needed, but 
only when that air is modeled by the *MAT_GAS_MIXTURE card. 
Example: 
Consider  a  tank  test  model  where  the  Lagrangian  tank  (Part  S1)  is  surrounded  by  an 
ALE  air  mesh  (Part  H4 = AMMGID  1).    There  are  2  ALE  parts  which  are  defined  but 
initially  have  no  corresponding  mesh:  part  5  (H5 = AMMGID  2)  is  the  resident  gas 
inside  the  tank  at  t = 0,  and  part  6  (H6 = AMMGID  2)  is  the  inflator  gas(es)  which  is 
injected into the tank when t > 0.  AMMGID stands for ALE Multi-Material Group ID.  
Please see figure and input below.  The *MAT_GAS_MIXTURE (MGM) card defines the 
gas properties of ALE parts H5 & H6.  The MGM card input for both method (A) and 
(B) are shown.
The  *INITIAL_GAS_MIXTURE  card  is  also  shown.    It  basically  specifies  that  “AM-
MGID 2 may be present in part or mesh H4 at t = 0, and the initial density of this gas is 
defined in the rho1 position which corresponds to the 1st material in the mixture (or H5, 
the resident gas).” 
Example configuration: 
Cut-off view 
S1 = tank 
H4 = AMMG1 = background 
outside  air  (initially  defined 
ALE mesh) 
H5 = AMMG2 = initial 
gas 
inside  the  tank  (this  has  no 
initial mesh)
H6 = AMMG2 = inflator 
gas(es) 
injected  in  (this  has  no  initial 
mesh)
Sample input: 
$------------------------------------------------------------------------------- 
*PART 
H5 = initial gas inside the tank 
$      PID     SECID       MID     EOSID      HGID      GRAV    ADPOPT      TMID 
         5         5         5         0         5         0         0 
*SECTION_SOLID 
         5        11         0 
$------------------------------------------------------------------------------- 
$ Example 1:  Constant heat capacities using per-mass unit. 
$*MAT_GAS_MIXTURE 
$      MID    IADIAB    R_univ 
$        5         0         0  
$  Cv1_mas   Cv2_mas   Cv3_mas   Cv4_mas   Cv5_mas   Cv6_mas   Cv7_mas   Cv8_mas 
$718.7828911237.56228 
$  Cp1_mas   Cp2_mas   Cp3_mas   Cp4_mas   Cp5_mas   Cp6_mas   Cp7_mas   Cp8_mas 
$1007.00058 1606.1117 
$------------------------------------------------------------------------------- 
$ Example 2:  Variable heat capacities using per-mole unit. 
*MAT_GAS_MIXTURE 
$      MID    IADIAB    R_univ 
         5         0  8.314470 
$      MW1       MW2       MW3       MW4       MW5       MW6       MW7       MW8 
 0.0288479   0.02256 
$  Cp1_mol   Cp2_mol   Cp3_mol   Cp4_mol   Cp5_mol   Cp6_mol   Cp7_mol   Cp8_mol 
 29.049852  36.23388 
$       B1        B2        B3        B4        B5        B6        B7        B8 
  7.056E-3  0.132E-1 
$       C1        C2        C3        C4        C5        C6        C7        C8 
 -1.225E-6 -0.190E-5 
$------------------------------------------------------------------------------- 
$ One card is defined for each AMMG that will occupy some elements of a mesh set
*INITIAL_GAS_MIXTURE 
$      SID     STYPE     MMGID        T0 
         4         1         1    298.15 
$     RHO1      RHO2      RHO3      RHO4      RHO5      RHO6      RHO7      RHO8 
1.17913E-9 
*INITIAL_GAS_MIXTURE 
$      SID     STYPE     MMGID        T0 
         4         1         2    298.15 
$     RHO1      RHO2      RHO3      RHO4      RHO5      RHO6      RHO7      RHO8 
1.17913E-9 
$-------------------------------------------------------------------------------
*MAT_EMMI 
This is Material Type 151.  The Evolving Microstructural Model of Inelasticity (EMMI) 
is  a  temperature  and  rate-dependent  state  variable  model  developed  to  represent  the 
large deformation of metals under diverse loading conditions [Marin 2005].  This model 
is available for 3D solid elements, 2D solid elements and thick shell forms 3 and 5 . 
  Card 1 
1 
2 
Variable 
MID 
RHO 
Type 
A8 
  Card 2 
1 
F 
2 
Variable 
RGAS 
BVECT 
Type 
F 
  Card 3 
1 
F 
2 
3 
E 
F 
3 
D0 
F 
3 
4 
PR 
F 
4 
QD 
F 
4 
5 
6 
7 
8 
5 
CV 
F 
5 
6 
7 
8 
ADRAG 
BDRAG 
DMTHTA 
F 
6 
F 
7 
F 
8 
Variable 
DMPHI 
DNTHTA 
DNPHI 
THETA0 
THETAM 
BETA0 
BTHETA 
DMR 
Type 
F 
  Card 4 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
DNUC1 
DNUC2 
DNUC3 
DNUC4 
DM1 
DM2 
DM3 
DM4 
Type 
F 
  Card 5 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
DM5 
Q1ND 
Q2ND 
Q3ND 
Q4ND 
CALPHA 
CKAPPA 
C1 
Type 
F 
F 
F 
F 
F 
F 
F
1 
Variable 
C2ND 
Type 
F 
  Card 7 
1 
Variable 
C10 
Type 
F 
  Card 8 
1 
*MAT_151 
2 
C3 
F 
2 
A1 
F 
2 
3 
C4 
F 
3 
A2 
F 
3 
4 
C5 
F 
4 
A3 
F 
4 
5 
C6 
F 
5 
A4 
F 
5 
6 
7 
8 
C7ND 
C8ND 
C9ND 
F 
6 
F 
7 
F 
8 
A_XX 
A_YY 
A_ZZ 
F 
6 
F 
7 
F 
8 
Variable 
A_XY 
A_YZ 
A_XZ 
ALPHXX 
ALPHYY 
ALPHZZ 
ALPHXY 
ALPHYZ 
Type 
F 
  Card 9 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
ALPHXZ  DKAPPA 
PHI0 
PHICR 
DLBDAG 
FACTOR  RSWTCH  DMGOPT 
Type 
F 
  Card 10 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
DELASO  DIMPLO 
ATOL 
RTOL 
DINTER 
Type 
F 
F 
F 
F
*MAT_EMMI 
  Card 11 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RHO 
Material density. 
E 
PR 
Young’s modulus 
Poisson’s ratio 
RGAS 
universal gas constant. 
BVECT 
Burger’s vector 
D0 
QD 
CV 
pre-exponential diffusivity coefficient 
activation energy 
specific heat at constant volume 
ADRAG 
drag intercept 
BDRAG 
drag coefficient 
DMTHTA 
shear modulus temperature coefficient 
DMPHI 
shear modulus damage coefficient 
DNTHTA 
bulk modulus temperature coefficient 
DNPHI 
bulk modulus damage coefficient 
THETA0 
reference temperature 
THETAM 
melt temperature 
BETA0 
coefficient of thermal expansion at reference temperature
*MAT_151 
DESCRIPTION
BTHETA 
thermal expansion temperature coefficient 
DMR 
damage rate sensitivity parameter 
DNUC1 
nucleation coefficient 1 
DNUC2 
nucleation coefficient 2 
DNUC3 
nucleation coefficient 3 
DNUC4 
nucleation coefficient 4 
DM1 
DM2 
DM3 
DM4 
DM5 
Q1ND 
Q2ND 
Q3ND 
Q4ND 
coefficient of yield temperature dependence 
coefficient of yield temperature dependence 
coefficient of yield temperature dependence 
coefficient of yield temperature dependence 
coefficient of yield temperature dependence 
dimensionless activation energy for f 
dimensionless activation energy for rd 
dimensionless activation energy for Rd 
dimensionless activation energy Rs 
CALPHA 
coefficient for backstress alpha 
CKAPPA 
coefficient for internal stress kappa 
C1 
parameter for flow rule exponent n 
C2ND 
parameter for transition rate f 
C3 
C4 
C5 
C6 
parameter for alpha dynamic recovery rd 
parameter for alpha hardening h 
parameter for kappa dynamic recovery Rd 
parameter for kappa hardening H 
C7ND 
parameter kappa static recovery Rs
C8ND 
C9ND 
C10 
A1 
A2 
A3 
A4 
A_XX 
A_YY 
A_ZZ 
A_XY 
A_YZ 
A_XZ 
*MAT_EMMI 
DESCRIPTION
parameter for yield 
parameter for temperature dependence of flow rule exponent n 
parameter for static recovery (set = 1) 
plastic anisotropy parameter 
plastic anisotropy parameter 
plastic anisotropy parameter 
plastic anisotropy parameter 
initial structure tensor component 
initial structure tensor component 
initial structure tensor component 
initial structure tensor component 
initial structure tensor component 
initial structure tensor component 
ALPHXX 
initial backstress component 
ALPHYY 
initial backstress component 
ALPHZZ 
initial backstress component 
ALPHXY 
initial backstress component 
ALPHYZ 
initial backstress component 
ALPHXZ 
initial backstress component 
DKAPPA 
initial isotropic internal stress 
PHI0 
initial isotropic porosity 
PHICR 
critical cutoff porosity 
DLBDAG 
slip system geometry parameter 
FACTOR 
fraction of plastic work converted to heat, adiabatic
*MAT_151 
DESCRIPTION
RSWTCH 
rate sensitivity switch 
DMGOPT 
Damage model option parameter 
EQ.1.0: pressure independent Cocks/Ashby 1980 
EQ.2.0: pressure dependent Cocks/Ashby 1980 
EQ.3.0: pressure dependent Cocks 1989 
DELASO 
Temperature option 
EQ.0.0: driven externally 
EQ.1.0: adiabatic 
DIMPLO 
Implementation option flag 
EQ.1.0: combined  viscous  drag  and 
thermally  activated
dislocation motion 
EQ.2.0: separate  viscous  drag  and 
thermally  activated
dislocation motion 
ATOL 
RTOL 
absolute error tolerance for local Newton iteration 
relative error tolerance for local Newton iteration 
DNITER 
maximum number of iterations for local Newton iteration 
Remarks: 
∇
= ℎ 𝐝𝑝 − 𝑟𝑑 𝜀̅
̇𝑝𝛼̅ 𝛂 
̇𝑝 − 𝑅𝑠𝜅sinh(𝑄𝑠𝜅) 
𝜅̇ = (𝐻 − 𝑅𝑑𝜅)𝜀̅
𝐝p = √
 𝜀̅
̇𝑝𝐧, 𝜀̅
̇𝑝 = 𝑓sinh𝑛 [⟨
𝜎̅̅̅̅̅
𝜅 + 𝑌
− 1⟩]
̇𝑝 − equation 
𝜀̅
𝑓 = 𝑐2exp (
𝑄1
) 
𝑛 =
𝑐9
− 𝑐1 
𝑌 = 𝑐8𝑌̂(𝜃) 
𝛂 − equation
𝜅 − equation
𝑟𝑑 = 𝑐3exp (
−𝑄2
)
𝑅𝑑 = 𝑐5exp (
−𝑄3
)
ℎ = 𝑐4𝜇̂(𝜃)
𝐻 = 𝑐6𝜇̂(𝜃)
𝑅𝑠 = 𝑐7exp (
−𝑄4
)
𝑄𝑠 = 𝑐10exp (
−𝑄5
)
Table M151-1.  Plasticity Material Functions of EMMI Model. 
Void growth: 
𝜑̇ =
√2
(1 − 𝜑)𝐺̂(𝜎̅̅̅̅̅𝑒𝑞, 𝑝̅, 𝜑)𝜀̅
̇𝑝 
𝐺̂(𝜎̅̅̅̅̅𝑒𝑞, 𝑝̅𝜏, 𝜑) =
√3
[
(1 − 𝜑)𝑚 + 1
− 1] sinh [
2(2𝑚 − 1)
2𝑚 + 1
⟨𝑝̅⟩
𝜎̅̅̅̅̅𝑒𝑞
]
*MAT_153 
This  is  Material  Type  153.  This  model  has  two  back  stress  terms  for  kinematic 
hardening  combined  with  isotropic  hardening  and  a  damage  model  for  modeling  low 
cycle  fatigue  and  failure.    Huang  [2006]  programmed  this  model  and  provided  it  as  a 
user subroutine with the documentation that follows.  It is available for beam, shell and 
solid elements.   
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
E 
F 
3 
4 
PR 
F 
4 
5 
6 
7 
8 
SIGY 
HARDI 
BETA 
LCSS 
F 
5 
F 
6 
F 
7 
I 
8 
Variable 
HARDK1  GAMMA1  HARDK2  GAMMA2
SRC 
SRP 
HARDK3  GAMMA3
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
F 
4 
Variable 
IDAM 
IDS 
IDEP 
EPSD 
Type 
I 
I 
I 
F 
F 
8 
F 
5 
S 
F 
F 
6 
T 
F 
F 
7 
DC 
F 
Optional Card 4 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
HARDK4  GAMMA4 
Type 
F
MID 
RO 
E 
PR 
*MAT_DAMAGE_3 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density, 𝜌 
Young’s modulus, E 
Poisson’s ratio, 𝑣 
SIGY 
Initial yield stress, 𝜎𝑦0 (ignored if LCSS.GT.0) 
HARDI 
Isotropic hardening modulus, H (ignored if LCSS.GT.0) 
BETA 
LCSS 
Isotropic  hardening  parameter,  𝛽.  Set  𝛽 = 0  for  linear  isotropic 
hardening.  (Ignored if LCSS.GT.0 or if HARDI.EQ.0.) 
Load curve ID defining effective stress vs.  effective plastic strain
for isotropic hardening.  The first abscissa value must be 
zero corresponding to the initial yield stress.  The first ordinate 
value is the initial yield stress.  
HARDK1 
Kinematic hardening modulus 𝐶1 
GAMMA1 
Kinematic hardening parameter 𝛾1.  Set 𝛾1 = 0 for linear 
kinematic hardening.  Ignored if (HARDK1.EQ.0) is defined. 
HARDK2 
Kinematic hardening modulus 𝐶2 
GAMMA2 
SRC 
SRP 
Kinematic hardening parameter 𝛾2
kinematic hardening.  Ignored if (HARDK2.EQ.0) is defined. 
Set 𝛾2 = 0 for linear 
.
Strain rate parameter, C, for Cowper Symonds strain rate model,
see below.  If zero, rate effects are not considered. 
Strain rate parameter, P, for Cowper Symonds strain rate model,
see below.  If zero, rate effects are not considered. 
HARDK3 
Kinematic hardening modulus 𝐶3 
GAMMA3 
Kinematic hardening parameter 𝛾3
kinematic hardening.  Ignored if (HARDK3.EQ.0) is defined. 
Set 𝛾3 = 0 for linear 
.
VARIABLE   
DESCRIPTION
IDAM 
Isotropic damage flag 
EQ.0: damage  is  inactivated.    IDS,  IDEP,  EPSD,  S,  T,  DC  are
ignored. 
EQ.1: damage is activated 
IDS 
Output stress flag 
EQ.0: undamaged stress is 𝜎̃  output 
EQ.1: damaged stress is 𝜎̃ (1 − 𝐷) output 
IDEP 
Damaged plastic strain 
EQ.0: plastic strain is accumulated 𝑟 = ∫ 𝜀̅
̇𝑝𝑙
EQ.1: damaged plastic strain is accumulated 𝑟 = ∫(1 − 𝐷)𝜀̅
̇𝑝𝑙 
EPSD 
Damage threshold 𝑟𝑑.  Damage accumulation begins when 𝑟 > 𝑟𝑑 
S 
T 
DC 
Damage material constant S.  Default = 𝜎𝑦0 200
⁄
Damage material constant t.  Default = 1 
Critical  damage  value  𝐷𝑐.    When  damage  value  reaches  critical, 
the element is deleted from calculation.  Default = 0.5 
HARDK4 
Kinematic hardening modulus 𝐶4  
Kinematic hardening parameter 𝛾4
kinematic hardening.  Ignored if (HARDK4.EQ.0) is defined. 
Set 𝛾4 = 0 for linear 
.
GAMMA4 
Remarks: 
This model is based on the work of Lemaitre [1992], and Dufailly and Lemaitre [1995].  
It  is  a  pressure-independent  plasticity  model  with  the  yield  surface  defined  by  the 
function 
where 𝜎𝑣 is uniaxial yield stress 
𝐹 = 𝜎̅̅̅̅̅ − 𝜎𝑦 = 0 
𝜎𝑦 = 𝜎𝑦0 +
[1 − exp(−𝛽𝑟)] 
By setting 𝛽 = 0, a linear isotropic hardening is obtained 
𝜎𝑦 = 𝜎𝑦0 + 𝐻𝑟
where  𝜎𝑣0  s  the  initial  yield  stress.    And  𝜎̅̅̅̅̅  is  the  equivalent  von  Mises  stress,  with 
respect to the deviatoric effective stress 
where s is deviatoric stress and α is the back stress, which is decomposed into several 
components 
se = 𝑑𝑒𝑣[σ̃] − α = s − α 
and  σ̃  is  effective  stress  (undamaged  stress),  based  on  Continuum  Damage  Mechanics 
model [Lemaitre 1992] 
α = ∑ αj
σ̃ =
1 − 𝐷
where D is the isotropic damage scalar, which is bounded by 0 and 1 
0 ≤ 𝐷 ≤ 1 
D = 0  represents  a  damage-free  material  RVE  (representative  volume  element),  while 
D = 1 represents a fully broken material RVE in two parts.  In fact, fracture occurs when 
𝐷 = 𝐷𝑐 < 1, modeled as element removal.  The evolution of the isotropic damage value 
related to ductile damage and fracture (the case where the plastic strain or dissipation is 
much larger than the elastic one, [Lemaitre 1992]) is defined as 
𝐷̇ =
⎧
{
⎨
{
⎩
)
(
̇pl
𝜀̅
𝑟 > 𝑟𝑑&
𝜎𝑚
𝜎eq
otherwise
> −
where 
𝜎𝑚
𝜎𝑒𝑞
 is the stress triaxiality, 𝑟𝑑 is damage threshold, S is a material constant, and Y 
is strain energy density release rate. 
𝑌 =
εel: 𝐃el: εel 
Where  𝐃el  represents  the  fourth-order  elasticity  tensor,  εel  is  elastic  strain.    And  t  is  a 
material  constant,  introduced  by  Dufailly  and  Lemaitre  [1995],  to  provide  additional 
degree  of  freedom  for  modeling  low-cycle  fatigue  (𝑡 = 1  in  Lemaitre  [1992]).    Dufailly 
and Lemaitre [1995] also proposed a simplified method to fit experimental results and 
get S and t. 
The equivalent Mises stress is defined as 
𝜎̅̅̅̅̅(s𝑒) = √
s𝑒: s𝑒 = √
∥s𝑒∥ 
The model assumes associated plastic flow 
ε̇pl =
∂𝐹
∂σ
𝑑𝜆 =
s𝑒
𝜎̅̅̅̅̅
𝑑𝜆
Where  𝑑𝜆  is  the  plastic  consistency  parameter.    The  evolution  of  the  kinematic 
component of the model is defined as [Armstrong and Frederick 1966]:  
α̇𝑗 =
⎧
{{
⎨
{{
⎩
𝐶𝑗ε̇pl − 𝛾𝑗α𝑗𝜀̅
̇pl                           IDEP = 0
α̇𝑗 = (1 − 𝐷) (
𝐶𝑗ε̇pl − 𝛾𝑗α𝑗𝜀̅
̇pl)       IDEP = 1
The damaged plastic strain is accumulated as 
̇pl                   IDEP = 0
⎧𝑟 = ∫ 𝜀̅
{
{⎨
𝑟 = ∫(1 − 𝐷)𝜀̅
⎩
̇pl     IDEP = 1
where 𝜀̅
̇pl is the equivalent plastic strain rate 
where ε̇pl represents the rate of plastic flow. 
̇pl = √
𝜀̅
ε̇pl: ε̇pl 
Strain  rate  is  accounted  for  using  the  Cowper  and  Symonds  model  which  scales  the 
yield stress with the factor 
where 𝜀̇ is the strain rate. 
1 + (
𝑝⁄
)
𝜀̇
Table 153.1 shows the difference between MAT 153 and MAT 104/105.  MAT 153 is less 
computationally  expensive  than  MAT  104/105.    Kinematic  hardening,  which  already 
exists in MAT 103, is included in MAT 153, but not in MAT 104/105.
MAT 153 
MAT 104 
MAT 105 
Computational cost 
1.0 
3.0 
3.0 
Isotropic hardening  One component 
Two components  One component
Kinematic hardening 
Four components 
N/A 
N/A 
Output stress 
Damagedplastic strain 
Accumulation when 
Isotropic plasticity 
Anisotropic plasticity 
Isotropic damage 
Anisotropic damage 
IDS = 0  𝜎̃  
IDS = 1  𝜎̃ (1 − 𝐷)
IDEP = 0  
𝑟 = ∫ 𝜀̅
̇pl 
IDEP = 1  
𝑟 = ∫(1 − 𝐷)𝜀̅
̇pl 
𝜎𝑚
𝜎𝑒𝑞
> −
Yes 
No 
Yes 
No 
𝜎̃ (1 − 𝐷) 
𝜎̃ (1 − 𝐷) 
𝑟 = ∫(1 − 𝐷)𝜀̅
̇pl 
𝑟 = ∫(1 − 𝐷)𝜀̅
̇pl 
𝜎1 > 0 
𝜎1 > 0 
Yes 
Yes 
Yes 
Yes 
Yes 
No 
Yes 
No 
Table M153-1.  Differences between MAT 153 and MAT 104/105
*MAT_DESHPANDE_FLECK_FOAM 
This  is  material  type  154  for  solid  elements.    This  material  is  for  modeling  aluminum 
foam used as a filler material in aluminum extrusions to enhance the energy absorbing 
capability  of  the  extrusion.    Such  energy  absorbers  are  used  in  vehicles  to  dissipate 
energy during impact.  This model was developed by Reyes, Hopperstad, Berstad, and 
Langseth [2002] and is based on the foam model by Deshpande and Fleck [2000]. 
  Card 1 
1 
2 
Variable 
MID 
RHO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
6 
7 
8 
ALPHA 
GAMMA 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EPSD 
ALPHA2 
BETA 
SIGP 
DERFI 
CFAIL 
PFAIL 
NUM 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RHO 
Mass density. 
E 
PR 
Young’s modulus. 
Poisson’s ratio. 
ALPHA 
Controls shape of yield surface. 
GAMMA 
See remarks. 
EPSD 
Densification strain.
*MAT_DESHPANDE_FLECK_FOAM 
DESCRIPTION
ALPHA2 
See remarks. 
BETA 
SIGP 
See remarks. 
See remarks. 
DERFI 
Type of derivation used in material subroutine 
EQ.0: Numerical derivation 
EQ.1: Analytical derivation 
Failure volumetric strain. 
Failure  principal  stress.    Must  be  sustained  NUM  (>0)  timesteps
to fail element. 
CFAIL 
PFAIL 
NUM 
Number of timesteps at or above PFAIL to trigger element failure.
Remarks: 
The yield stress function Φ is defined by: 
The equivalent stress 𝜎̂  is given by: 
Φ = 𝜎̂ − 𝜎𝑦 
𝜎̂ 2 =
𝜎𝑉𝑀
2 + 𝛼2𝜎𝑚
1 + (𝛼
)
where, 𝜎𝑉𝑀, is the von Mises effective stress: 
𝜎𝑉𝑀 = √
σdev: σdev 
In this equation 𝜎𝑚 and 𝜎 𝑑𝑒𝑣 are the mean and deviatoric stress: 
The yield stress 𝜎𝑦 can be expressed as: 
σdev = σ − 𝜎𝑚I 
𝜎𝑦 = 𝜎𝑝 + 𝛾
𝜀̂
𝜀𝐷
+ 𝛼2ln
⎡
⎢
1 − ( 𝜀̂
⎣
𝜀𝐷
⎤ 
⎥
⎦
)
Here,  𝜎𝑝,   𝛼2, 𝛾  and  𝛽  are  material  parameters.    The  densification  strain 𝜀𝐷  is  defined 
as:
𝜀𝐷 = −ln (
𝜌𝑓
𝜌𝑓0
) 
where 𝜌𝑓  is the foam density and 𝜌𝑓0 is the density of the virgin material.
*MAT_PLASTICITY_COMPRESSION_TENSION_EOS 
This  is  Material  Type  155.    An  isotropic  elastic-plastic  material  where  unique  yield 
stress  versus  plastic  strain  curves  can  be  defined  for  compression  and  tension.    Also, 
failure can occur based on a plastic strain or a minimum time step size.  Rate effects on 
the yield stress are modeled either by using the Cowper-Symonds strain rate model or 
by using two load curves that scale the yield stress values in compression and tension, 
respectively.    Material  rate  effects,  which  are  independent  of  the  plasticity  model,  are 
based on a 6-term Prony series Maxwell mode that generates an additional stress tensor.  
The  viscous  stress  tensor  is  superimposed  on  the  stress  tensor  generated  by  the 
plasticity.  Pressure is defined by an equation of state, which is required to utilize this 
model.  This model is applicable to solid elements and SPH. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
Default 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
5 
C 
F 
0 
5 
6 
P 
F 
0 
6 
7 
8 
FAIL 
TDEL 
F 
10.E+20 
7 
F 
0 
8 
Variable 
LCIDC 
LCIDT 
LCSRC 
LCSRT 
SRFLAG 
Type 
Default 
  Card 3 
Variable 
Type 
Default 
I 
0 
1 
PC 
F 
0 
I 
0 
2 
PT 
F 
0 
I 
0 
3 
I 
0 
4 
F 
0 
5 
6 
7 
8 
PCUTC 
PCUTT 
PCUTF 
SCALEP 
SCALEE 
F 
0 
F 
0 
F 
0 
F 
0 
F
2 
3 
4 
5 
6 
7 
8 
  Card 4 
Variable 
Type 
1 
K 
F 
Viscoelastic Constant Cards.  Card Format for viscoelastic constants.  Up to 6 cards 
may  be  input.    A  keyword  card  (with  a  “*”  in  column  1)  terminates  this  input  if  less 
than 6 cards are used.   
 Optional 
Variable 
Type 
1 
GI 
F 
  VARIABLE   
MID 
RO 
E 
PR 
C 
P 
2 
3 
4 
5 
6 
7 
8 
BETAI 
F 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
Strain rate parameter, C, see formula below. 
Strain rate parameter, P, see formula below. 
FAIL 
Failure flag. 
LT.0.0:  User defined failure subroutine, matusr_24 in dyn21.F, 
is called to determine failure 
EQ.0.0: Failure is not considered.  This option is recommended
if failure is not of interest since many calculations will 
be saved. 
GT.0.0:  Plastic strain to failure.  When the plastic strain reaches
this value, the element is deleted from the calculation. 
TDEL 
Minimum time step size for automatic element deletion.
LCIDC 
LCIDT 
LCSRC 
LCSRT 
*MAT_PLASTICITY_COMPRESSION_TENSION_EOS 
DESCRIPTION
Load curve ID defining yield stress versus effective plastic strain 
in compression. 
Load curve ID defining yield stress versus effective plastic strain
in tension. 
Optional load curve ID defining strain rate scaling effect on yield
stress when the material is in compression. 
Optional load curve ID defining strain rate scaling effect on yield
stress when the material is in tension. 
SRFLAG 
Formulation for rate effects: 
EQ.0.0: Total strain rate, 
EQ.1.0: Deviatoric strain rate. 
PC 
PT 
PCUTC 
PCUTT 
Compressive  mean  stress  (pressure)  at  which  the  yield  stress 
follows  load  curve  ID,  LCIDC.    If  the  pressure  falls  between  PC
and PT a weighted average of the two load curves is used. 
Tensile  mean  stress  at  which  the  yield  stress  follows  load  curve
ID, LCIDT. 
Pressure  cut-off  in  compression.    When  the  pressure  cut-off  is 
reached  the  deviatoric  stress  tensor  is  set  to  zero. 
  The
compressive  pressure  is  not,  however,  limited  to  PCUTC.    Like
the yield stress, PCUTC is scaled to account for rate effects. 
Pressure cut-off in tension.  When the pressure cut-off is reached 
the  deviatoric  stress  tensor  and  tensile  pressure  is  set  to  zero.
Like the yield stress, PCUTT is scaled to account for rate effects. 
PCUTF 
Pressure cut-off flag. 
EQ.0.0: Inactive, 
EQ.1.0: Active. 
SCALEP 
Scale factor applied to the yield stress after the pressure cut-off is 
reached  in  either  compression  or  tension. 
  If  SCALEP = 0 
(default),  the  deviatoric  stress  is  set  to  zero  after  the  cut-off  is 
reached.
VARIABLE   
SCALEE 
K 
GI 
DESCRIPTION
Scale factor applied to the yield stress after the strain exceeds the 
failure strain set by FAIL.  If SCALEE = 0 (default), the deviatoric 
strain  is  set  to  zero  if  the  failure  strain  is  exceeded.    IF  both
SCALEP > 0 and SCALEE > 0 and both failure conditions are met, 
then the minimum scale factor is used. 
Optional bulk modulus for the viscoelastic material.  If nonzero a
Kelvin type behavior will be obtained.  Generally, K is set to zero.
Optional shear relaxation modulus for the ith term 
BETAI 
Optional shear decay constant for the ith term 
Remarks: 
The  stress  strain  behavior  follows  a  different  curve  in  compression  than  it  does  in 
tension.    Tension  is  determined  by  the  sign  of  the  mean  stress  where  a  positive  mean 
stress  (i.e.,  a  negative  pressure)  is  indicative  of  tension.    Two  curves  must  be  defined 
giving  the  yield  stress  versus  effective  plastic  strain  for  both  the  tension  and 
compression regimes. 
Mean  stress  is  an  invariant  which  can  be  expressed  as  (σx  +  σy  +  σz)/3.    PC  and  PT 
define  a  range  of  mean  stress  values  within  which  interpolation  is  done  between  the 
tensile  yield  surface  and  compressive  yield  surface.      PC  and  PT  are  not  true  material 
properties  but  are  just  a  numerical  convenience  so  that  the  transition  from  one  yield 
surface to the other is not abrupt as the sign of the mean stress changes.  Both PC and 
PT  are  input  as  positive  values  as  it  is  implied  that  PC  is  a  compressive  mean  stress 
value and PT is tensile mean stress value. 
Strain  rate  may  be  accounted  for  using  the  Cowper  and  Symonds  model  which  scales 
the yield stress with the factor: 
where 𝜀̇ is the strain rate, 
1 + (
𝑝⁄
)
𝜀̇
𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗.
*MAT_PLASTICITY_COMPRESSION_TENSION_EOS 
History Variable 
Description 
4 
5 
6 
7 
Tensile  pressure  cutoff  (set  to  zero  if 
tensile or compressive failure occurs) 
The cutoff flag, initially equals 1, set to 
0  if  tensile  or  compressive  failure 
occurs 
The failure mode flag 
EQ.0:  if no failure 
EQ.1:  if compressive failure 
EQ.2:  if tensile failure 
EQ.3:  if failure by plastic strain 
The current flow stress
*MAT_156 
This is material type 156 for truss elements.  This material is a Hill-type muscle model 
with  activation  and  a  parallel  damper.    Also,  see  *MAT_SPRING_MUSCLE  where  a 
description of the theory is available. 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
4 
5 
6 
7 
8 
SNO 
SRM 
PIS 
SSM 
CER 
DMP 
Type 
A8 
F 
F 
F 
F 
F 
F 
F 
Default 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ALM 
SFR 
SVS 
SVR 
SSP 
Type 
F 
F 
F 
F 
F 
Default 
0.0 
1.0 
1.0 
1.0 
0.0 
  VARIABLE   
DESCRIPTION
MID 
RO 
SNO 
SRM 
PIS 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Material density in the initial undeformed configuration. 
Initial  stretch  ratio, 
𝑙0
𝑙orig
,  i.e.,  the  length  as  defined  by  the  nodal 
points at t = 0 divided by the original initial length.  The density
for the nodal mass calculation is RO/SNO, or 
𝑙orig
𝑙0
𝜌. 
Maximum strain rate. 
Peak isometric stress corresponding to the dimensionless value of
unity  in  the  dimensionless  stress  versus  strain  function,  see  SSP
below.
SSM 
CER 
DMP 
ALM 
*MAT_MUSCLE 
DESCRIPTION
Strain  when  the  dimensionless  stress  versus  strain  function,  SSP
below, reaches its maximum stress value. 
Constant,  governing  the  exponential  rise  of  SSP.    Required  if
SSP = 0. 
Damping constant (stress × time units). 
Activation level vs.  time. 
LT.0:  absolute value gives load curve ID 
GE.0: constant value of ALM is used 
SFR 
Scale factor for strain rate maximum vs.  activation level, 𝑎(𝑡). 
LT.0:  absolute value gives load curve ID 
GE.0: constant value of 1.0 is used 
SVS 
SVR 
Active dimensionless tensile stress vs.  the stretch ratio, 
𝑙orig
. 
LT.0:  absolute value gives load curve ID 
GE.0: constant value of 1.0 is used 
Active dimensionless tensile stress vs.  the normalized strain rate,
̇. 
𝜀̅
LT.0:  absolute value gives load curve ID 
GE.0: constant value of 1.0 is used 
SSP 
Isometric  dimensionless  stress  vs.    the  stretch  ratio, 
𝑙orig
  for  the 
parallel elastic element. 
LT.0:  absolute value gives load curve ID or table ID 
EQ.0: exponential function is used  
GT.0: constant value of 0.0 is used 
Remarks: 
The  material  behavior  of  the  muscle  model  is  adapted  from  *MAT_S15,  the  spring 
muscle  model  and  treated  here  as  a  standard  material.    The  initial  length  of  muscle  is 
calculated automatically.  The force, relative length and shortening velocity are replaced 
by stress, strain and strain rate.  A new parallel damping element is added.
The strain 𝜀 and normalized strain rate 𝜀̅
̇ are defined respectively as 
and, 
𝜀 =
𝑙orig
− 1 
= SNO ×
𝑙0
− 1 
𝜀̅
̇ =
𝑙orig
𝜀̇
𝜀̇max
= SNO ×
𝑙0
×
𝜀̇
SFR × SRM
where  𝜀̇ = ∆𝜀/∆𝑡  (current  strain  increment  divided  by  current  time  step),  l = current 
muscle length, and 𝑙orig = original muscle length. 
From the relation above, it is known: 
𝑙orig =
𝑙0
1 + 𝜀0
where 𝜀0 = SNO − 1 and 𝑙0 = muscle length at time 0. 
Stress of Contractile Element is: 
𝜎1 = 𝜎max𝑎(𝑡)𝑓 (
𝑙orig
) 𝑔(𝜀̅
̇) 
where 𝜎max = PIS, 𝑎(𝑡) = ALM, 𝑓 (𝑙/𝑙orig) = SVS, and 𝑔(𝜀̅
̇) = SVR. 
Stress of Passive Element is: 
𝜎2 =
⎧
{{{
⎨
{{{
⎩
𝜎maxℎ (
̇,
𝜎maxℎ (𝜀̅
)
𝑙orig
𝑙orig
for curve
) for table
where ℎ = SSP.  For SSP < 0, the absolute value gives a load curve ID or table ID.  The 
load curve defines isometric dimensionless stress ℎ versus stretch ratio 𝑙/𝑙orig. The table 
̇  a  load  curve  giving  the  isometric  dimension-
defines  for  each  normalized  strain  rate 𝜀̅
less stress ℎ versus stretch ratio 𝑙/𝑙orig for that rate.
*MAT_MUSCLE 
⎜⎜⎜⎜⎛
⎝
⁄
𝑙orig
=
⎟⎟⎟⎟⎞
⎠
exp(CER) − 1
⎧0
{
{
{
{
{
{
⎨
{
{
{
{
{
{
⎩
SSM
⁄ < 1
𝑙orig
[ exp (
CER
SSM
𝜀) − 1]
⁄ ≥ 1 CER ≠ 0
𝑙orig
⁄ ≥ 1 CER = 0
𝑙orig
Stress of Damping Element is: 
Total Stress is: 
σ3 = DMP ×
𝑙orig
 ε̇ 
𝜎 = 𝜎1 + 𝜎2 + 𝜎3
*MAT_ANISOTROPIC_ELASTIC_PLASTIC 
This  is  Material  Type  157.    This  material  model  is  a  combination  of  the  anisotropic 
elastic  material  model  (MAT_002)  and  the  anisotropic  plastic  material  model  (MAT_-
103_P).  Also, brittle orthotropic failure based on a phenomenological Tsai-Wu criterion 
can be defined. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
4 
5 
6 
7 
8 
SIGY 
LCSS 
QR1 
CR1 
QR2 
CR2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
C11 
C12 
C13 
C14 
C15 
C16 
C22 
C23 
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
C24 
C25 
C26 
C33 
C34 
C35 
C36 
C44 
Type 
F 
  Card 4 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
C45 
C46 
C55 
C56 
C66 
R00 or F  R45 or G  R90 or H 
Type 
F 
  Card 5 
1 
F 
2 
F 
3 
F 
4 
F 
5 
Variable 
S11 or L  S22 or M  S33 or N 
S12 
AOPT 
Type 
F 
F 
F 
F 
F 
F 
6 
VP 
F 
F 
7 
F 
8 
MACF
Variable 
1 
XP 
Type 
F 
  Card 7 
Variable 
1 
V1 
Type 
F 
*MAT_ANISOTROPIC_ELASTIC_PLASTIC 
2 
YP 
F 
2 
V2 
F 
3 
ZP 
F 
3 
V3 
F 
4 
A1 
F 
4 
D1 
F 
5 
A2 
F 
5 
D2 
F 
6 
A3 
F 
6 
D3 
F 
7 
8 
EXTRA 
F 
8 
7 
BETA 
IHIS 
F 
F 
Two additional cards for EXTRA = 1 or 2. 
  Card 8 
Variable 
1 
XT 
Type 
F 
  Card 9 
Variable 
1 
ZT 
Type 
F 
2 
XC 
F 
2 
ZC 
F 
3 
YT 
F 
3 
4 
YC 
F 
4 
5 
6 
7 
8 
SXY 
FF12 
NCFAIL 
F 
5 
F 
6 
7 
F 
8 
SYZ 
SZX 
FF23 
FF31 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
SIGY 
LCSS 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Initial yield stress 
Load curve ID or Table ID. 
Load  Curve.    When  LCSS  is  a  Load  curve  ID,  it  is  taken  as
defining effective stress versus effective plastic strain.  If defined
VARIABLE   
DESCRIPTION
QR1, CR1, QR2, and CR2 are ignored. 
Tabular  Data.    The  table  ID  defines  for  each  strain  rate  value  a
load  curve  ID  giving  the  stress  versus  effective  plastic  strain  for 
that rate, See Figure M24-1.  When the strain rate falls below the 
minimum value, the stress versus effective plastic strain curve for
the lowest value of strain rate is used.  Likewise, when the strain 
rate exceeds the maximum value the stress versus effective plastic
strain curve for the highest value of strain rate is used.  
Logarithmically Defined Tables.  If the first stress-strain curve in 
the table corresponds to a negative strain rate, LS-DYNA assumes 
that  the  natural  logarithm  of  the  strain  rate  value  is  used  for  all
stress-strain curves.   Since the tables are internally discretized to
equally  space  the  points,  natural  logarithms  are  necessary,  for
example,  if  the  curves  correspond  to  rates  from  10−4  to  104. 
Computing  natural  logarithms  can  substantially  increase  the
computational time on certain computer architectures. 
Isotropic hardening parameter 
Isotropic hardening parameter 
Isotropic hardening parameter 
Isotropic hardening parameter 
The i, j term in the 6 × 6 anisotropic constitutive matrix.  Note that 
1  corresponds  to  the  a  material  direction,  2  to  the  b  material 
direction, and 3 to the c material direction. 
𝑅00 for shell 
(Default = 1.0) 
𝑅45 for shell 
(Default = 1.0) 
𝑅90 for shell 
(Default = 1.0) 
𝐹 for brick 
(Default = 1 2⁄ ) 
𝐺 for brick 
(Default = 1 2⁄ ) 
𝐻 for brick 
(Default = 1 2⁄ ) 
𝐿 for brick 
(Default = 3 2⁄ ) 
𝑀 for brick 
(Default = 3 2⁄ ) 
QR1 
CR1 
QR2 
CR2 
Cij 
R00 
R45 
R90 
F 
G 
H 
L
N 
S11 
S22 
S33 
S12 
*MAT_ANISOTROPIC_ELASTIC_PLASTIC 
DESCRIPTION
𝑁 for brick 
(Default = 3 2⁄ ) 
Yield stress in local-x direction (shells only).  This input is ignored 
when 
R00, R45, R90 > 0.
Yield stress in local-y direction (shells only).  This input is ignored 
when 
R00, R45, R90 > 0. 
Yield stress in local-z direction (shells only).  This input is ignored 
when 
R00, R45, R90 > 0. 
Yield  stress  in  local-xy  direction  (shells  only).    This  input  is 
ignored when 
R00, R45, R90 > 0. 
AOPT 
Material  axes  option  .  Available in R3 version of 971 
and later.
VARIABLE   
DESCRIPTION
VP 
Formulation for rate effects:  
EQ.0.0: scale yield stress (default), 
EQ.1.0:  viscoplastic formulation. 
MACF 
Material axes change flag for brick elements: 
EQ.1: No change, default, 
EQ.2: switch material axes 𝑎 and 𝑏, 
EQ.3: switch material axes 𝑎 and 𝑐, 
EQ.4: switch material axes 𝑏 and 𝑐. 
XP, YP, ZP 
coordinates of point 𝐩 for AOPT = 1 and 4. 
A1, A2, A3 
components of vector 𝐚 for AOPT = 2. 
D1, D2, D3 
components of vector 𝐝 for AOPT = 2. 
V1, V2, V3 
components of vector 𝐯 for AOPT = 3 and 4. 
BETA 
Material  angle  in  degrees  for  AOPT = 0  (shells  only)  and 
AOPT = 3.      BETA  may  be  overridden  on  the  element  card,  see
*ELEMENT_SHELL_BETA and *ELEMENT_SOLID_ORTHO. 
IHIS 
Flag for material properties initialization. 
EQ.0: material properties defined in Cards 1-5 are used 
GE.1: Use 
*INITIAL_STRESS_SOLID/SHELL 
initialize 
material  properties  on  an  element-by-element  basis  for 
solid or shell elements, respectively .
to 
EXTRA 
Flag to input further data : 
EQ.1.0: Tsai-Wu failure criterion parameters (cards 8 and 9) 
EQ.2.0: Tsai-Hill failure criterion parameters (cards 8 and 9) 
XT 
Longitudinal tensile strength, a-axis. 
GT.0.0:  constant value  
LT.0.0:  Load  curve  ID = (-XT)  which  defines  the  longitudinal 
tensile  strength  vs.    strain  rate.    If  the  first  strain  rate
value  in  the  curve  is  negative,  it  is  assumed  that  all
strain rate values are given as natural logarithm of the
strain rate.
*MAT_ANISOTROPIC_ELASTIC_PLASTIC 
DESCRIPTION
XC 
Longitudinal compressive strength, a-axis (positive value).  
GT.0.0:  constant value  
LT.0.0:  Load  curve  ID = (-XC)  which  defines  the  longitudinal 
compressive strength vs.  strain rate.  If the first strain
rate value in the curve is negative, it is assumed that all
strain rate values are given as natural logarithm of the
strain rate. 
YT 
Transverse tensile strength, b-axis.  
GT.0.0:  constant value  
LT.0.0:  Load  curve  ID = (-YT)  which  defines  the  transverse 
tensile  strength  vs.    strain  rate.    If  the  first  strain  rate
value  in  the  curve  is  negative,  it  is  assumed  that  all
strain rate values are given as natural logarithm of the
strain rate. 
YC 
Transverse compressive strength, b-axis (positive value). 
GT.0.0:  constant value  
LT.0.0:  Load  curve  ID = (-YC)  which  defines  the  transverse 
compressive strength vs.  strain rate.  If the first strain
rate value in the curve is negative, it is assumed that all
strain rate values are given as natural logarithm of the
strain rate. 
SXY 
Shear strength, ab-plane. 
GT.0.0:  constant value  
LT.0.0:  Load  curve  ID = (-SXY)  which  defines  the  shear 
strength vs.  strain rate.  If the first strain rate value in
the  curve  is  negative,  it  is  assumed  that  all  strain  rate
values are given as natural logarithm of the strain rate.
FF12 
NCFAIL 
Scale  factor  between  -1  and  +1  for  interaction  term  F12,  see 
Remarks. 
Number of timesteps to reduce stresses until element deletion. 
The default is NCFAIL = 10.
VARIABLE   
DESCRIPTION
ZT 
Transverse tensile strength, c-axis (solid elements only). 
GT.0.0:  constant value  
LT.0.0:  Load  curve  ID = (-ZT)  which  defines  the  transverse 
tensile  strength  vs.    strain  rate.    If  the  first  strain  rate
value  in  the  curve  is  negative,  it  is  assumed  that  all
strain rate values are given as natural logarithm of the
strain rate. 
ZC 
Transverse compressive strength, c-axis (positive value)  
(solid elements only).  
GT.0.0:  constant value  
LT.0.0:  Load  curve  ID = (-ZC)  which  defines  the  transverse 
compressive strength vs.  strain rate.  If the first strain
rate value in the curve is negative, it is assumed that all 
strain rate values are given as natural logarithm of the
strain rate. 
SYZ 
Shear strength, bc-plane (solid elements only).  
GT.0.0:  constant value  
LT.0.0:  Load  curve  ID = (-SYZ)  which  defines  the  shear 
strength vs.  strain rate.  If the first strain rate value in
the  curve  is  negative,  it  is  assumed  that  all  strain  rate
values are given as natural logarithm of the strain rate.
SZX 
Shear strength, ca-plane (solid elements only).  
GT.0.0:  constant value  
LT.0.0:  Load  curve  ID = (-SZX)  which  defines  the  shear 
strength vs.  strain rate.  If the first strain rate value in
the  curve  is  negative,  it  is  assumed  that  all  strain  rate
values are given as natural logarithm of the strain rate.
FF23 
FF31 
Scale  factor  between  -1  and  +1  for  interaction  term  F23,  see 
Remarks 
(solid elements only). 
Scale  factor  between  -1  and  +1  for  interaction  term  F31,  see 
Remarks  
(solid elements only).
Description of IHIS (Solid Elements): 
Several  of  this  material’s  parameters  may  be  overwritten  on  an  element-by-element 
basis through history variables using the *INITIAL_STRESS_SOLID keyword.  Bitwise 
(binary) expansion of IHIS determines which material properties are to be read: 
IHIS = 𝑎3 × 8 + 𝑎2 × 4 + 𝑎1 × 2 + 𝑎0, 
where each 𝑎𝑖 is a binary flag set to either 1 or 0.  The 𝑎𝑖 are interpreted according to the 
following table. 
Flag 
Description 
Variables 
𝑎0  Material directions 
𝑞11, 𝑞12, 𝑞13, 𝑞31, 𝑞32, 𝑞33 
𝑎1 
𝑎2 
𝑎3 
Anisotropic stiffness 
Cij 
Anisotropic constants 
F, G, H, L, M, N 
Stress-strain Curve 
LCSS 
# 
6 
21 
6 
1 
The  NHISV  field  on  *INITIAL_STRESS_SOLID  must  be  set  equal  to  the  sum  of  the 
number of variables to be read in, which depends on IHIS (and the 𝑎𝑖): 
NHISV = 6𝑎0 + 21𝑎1 + 6𝑎2 + 𝑎3. 
Then, in the following order, *INITIAL_STRESS_SOLID processes the history variables, 
HISVi,  as: 
1. 
2. 
3. 
4. 
6 material direction parameters when 𝑎0 = 1 
21 anisotropic stiffness parameters when 𝑎1 = 1 
6 anisotropic constants when 𝑎2 = 1 
1 parameters when 𝑎3 = 1 
The 𝑞𝑖𝑗 terms are the first and third rows of a rotation matrix for the rotation from a co-
rotational  element’s  system  and  the  𝑎-𝑏-𝑐  material  directions.    The  𝑐𝑖𝑗  terms  are  the 
upper  triangular  terms  of  the  symmetric  stiffness  matrix,  𝑐11,  𝑐12,  𝑐13,  𝑐14,  𝑐15,  𝑐16,  𝑐22, 
𝑐23, 𝑐24, 𝑐25, 𝑐26, 𝑐33, 𝑐34, 𝑐35, 𝑐36, 𝑐44, 𝑐45, 𝑐46, 𝑐55, 𝑐56, and 𝑐66. 
Description of IHIS (Shell Elements): 
Several  of  this  material’s  parameters  may  be  overwritten  on  an  element-by-element 
basis through history variables using the *INITIAL_STRESS_SHELL keyword.  Bitwise 
(binary) expansion of IHIS determines which material properties are to be read: 
IHIS = 𝑎4 × 16 + 𝑎3 × 8 + 𝑎2 × 4 + 𝑎1 × 2 + 𝑎0, 
where each 𝑎𝑖 is a binary flag set to either 1 or 0.  The 𝑎𝑖 are interpreted according to the 
following table.
Flag 
Description 
Variables 
𝑎0  Material directions 
Anisotropic stiffness 
𝑞1, 𝑞2 
Cij 
Anisotropic constants 
𝑟00, 𝑟45, 𝑟90 
Stress-strain Curve 
LCSS 
Strength limits 
XT, XC, YT, YC, SXY 
𝑎1 
𝑎2 
𝑎3 
𝑎4 
# 
2 
21 
3 
1 
5 
The  NHISV  field  on  *INITIAL_STRESS_SHELL  must  be  set  equal  to  the  sum  of  the 
number of variables to be read in, which depends on IHIS (and the 𝑎𝑖): 
NHISV = 2𝑎0 + 21𝑎1 + 3𝑎2 + 𝑎3 + 5𝑎4. 
Then, in the following order, *INITIAL_STRESS_SHELL processes the history variables, 
HISVi,  as: 
5. 
6. 
7. 
8. 
9. 
2 material direction parameters when 𝑎0 = 1 
21 anisotropic stiffness parameters when 𝑎1 = 1 
3 anisotropic constants when 𝑎2 = 1 
1 parameters when 𝑎3 = 1 
5 strength parameters when 𝑎4 = 1 
The  𝑞𝑖  terms  are  the  material  direction  cosine  and  sinus  for  the  rotation  from  a  co-
rotational element’s system to the 𝑎-𝑏-𝑐 material directions.  The 𝑐𝑖𝑗 terms are the upper 
triangular terms of the symmetric stiffness matrix, 𝑐11, 𝑐12, 𝑐13, 𝑐14, 𝑐15, 𝑐16, 𝑐22, 𝑐23, 𝑐24, 
𝑐25, 𝑐26, 𝑐33, 𝑐34, 𝑐35, 𝑐36, 𝑐44, 𝑐45, 𝑐46, 𝑐55, 𝑐56, and 𝑐66. 
Tsai-Wu failure criterion (EXTRA = 1): 
Brittle  failure  with  different  strengths  in tension  and  compression  in  all  main  material 
directions  can  be  invoked  with  EXTRA = 1  and  the  definition  of  corresponding 
parameters on Cards 8 and 9.  The model used is the phenomenological Tsai-Wu failure 
criterion which requires that  
+
XT ⋅ XC
(
−
−
XT
YC
) 𝜎𝑎𝑎 + (
XC
YT ⋅ YC
ZC
SYZ2 𝜎𝑏𝑐
+2 ⋅ 𝐹12 ⋅   𝜎𝑎𝑎𝜎𝑏𝑏 + 2 ⋅ 𝐹23 ⋅   𝜎𝑏𝑏𝜎𝑐𝑐 + 2 ⋅ 𝐹31 ⋅   𝜎𝑐𝑐𝜎𝑎𝑎 < 1 
YT
ZT ⋅ ZC
SXY2 𝜎𝑎𝑏
) 𝜎𝑏𝑏 + (
ZT
) 𝜎𝑐𝑐 
2 +
2 +
2 +
2 +
𝜎𝑏𝑏
𝜎𝑐𝑐
−
𝜎𝑎𝑎
2 +
2  
SZX2 𝜎𝑐𝑎
for the 3-dimensional case (solid elements) with three planes of symmetry with respect 
to the material coordinate system.  The interaction terms 𝐹12, 𝐹23, and 𝐹31 are given by
𝐹12 = FF12 ⋅ √
ZT⋅ZC⋅XT⋅XC 
For the 2-dimensional case of plane stress (shell elements) this expression reduces to: 
XT⋅XC⋅YT⋅YC ,    𝐹23 = FF23 ⋅ √
YT⋅YC⋅ZT⋅ZC ,    𝐹31 = FF31 ⋅ √
(
XT
−
XC
) 𝜎𝑎𝑎 + (
YC
) 𝜎𝑏𝑏 +
XT ⋅ XC
2 +
𝜎𝑎𝑎
YT ⋅ YC
2  
𝜎𝑏𝑏
−
YT
SXY2 𝜎𝑎𝑏
+
2 + 2 ⋅ 𝐹12 ⋅   𝜎𝑎𝑎𝜎𝑏𝑏 < 1 
If  these  conditions  are  violated,  then  the  stress  tensor  will  be  reduced  to  zero  over 
NCFAIL time steps and then the element gets eroded.  A small value for NCFAIL (< 50) 
is recommended to avoid unphysical behavior, the default is 10.  The default values for 
the  strengths  XT,  XC,  YT,  YC,  ZT,  ZC,  SXY,  SYZ,  and  SZX  are  1e20,  i.e.    basically  no 
limits.    The  scale  factors  FF12,  FF23,  and  FF31  for  the  interaction  terms  are  zero  by 
default.  
Tsai-Hill failure criterion (EXTRA = 2): 
Brittle  failure  with  different  strengths  in tension  and  compression  in  all  main  material 
directions  can  be  invoked  with  EXTRA = 2  and  the  definition  of  corresponding 
parameters  on  Cards  8  and  9  (FF12,  FF23  and  FF31  are  not  used  in  this  model).    The 
model based on the HILL criterion which can be written as 
(G + H)σaa
2 + (F + H)σbb
2 + 2Mσca
2 + (F + G)σcc
2 < 1 
2 + 2Lσbc
+2Nσab
2 − 2Hσaaσbb − 2F σbbσcc − 2Gσccσaa 
for the 3-dimensional case.  The constants H,F,G,N,L,M can be expressed in terms of the 
strength limits (which then becomes the TSAI-HILL criterion), where the current stress 
state  defines  whether  the  compressive  or  the  tensile  strength  limit  will  enter  into  the 
equation:
G + H =
2    ;   F + H =
Xi
2    ;   F + G =
Yi
2    ;   2𝑁 =
Zi
𝑆𝑋𝑌2    ;   2𝐿 =
𝑆𝑌𝑍2    ;   2𝑁
=
𝑆𝑍𝑋2 
2 − 1
2 + 1
2)   ;    G= 0.5 ⋅ ( 1
2 − 1
2 + 1
2)   ;   F= 0.5 ⋅ ( 1
2 − 1
2 + 1
H= 0.5 ⋅ ( 1
2) 
𝑌𝑖
𝑍𝑖
𝑋𝑖
𝑋𝑖
𝑍𝑖
𝑌𝑖
𝑍𝑖
𝑌𝑖
𝑋𝑖
𝑋𝑖 = {
𝑋𝑇      𝑖𝑓 𝜎𝑎𝑎 > 0
𝑋𝐶      𝑖𝑓 𝜎𝑎𝑎 < 0
    ;    𝑌𝑖 = {
𝑌𝑇      𝑖𝑓 𝜎𝑏𝑏 > 0
𝑌𝐶      𝑖𝑓 𝜎𝑏𝑏 < 0
   ;    𝑍𝑖 = {
𝑍𝑇      𝑖𝑓 𝜎𝑐𝑐 > 0
𝑍𝐶      𝑖𝑓 𝜎𝑐𝑐 < 0
For  the  2-dimensional  case  of  plane  stress  (shell  elements)  the  TSAI-HILL  criterion 
reduces to: 
(G + H)σaa
2 + (F + H)σbb
2 − 2Hσaaσbb + 2Nσab
2 < 1 
with 
G + H =
2    ;   F + H =
Xi
2    ;   H = 0.5 ⋅ (
Yi
2)  ;   2𝑁 =
Xi
𝑆𝑋𝑌2   
If  these  conditions  are  violated,  then  the  stress  tensor  will  be  reduced  to  zero  over 
NCFAIL time steps and then the element gets eroded.  A small value for NCFAIL (< 50) 
is recommended to avoid unphysical behavior, the default is 10.  The default values for 
the  strengths  XT,  XC,  YT,  YC,  ZT,  ZC,  SXY,  SYZ,  and  SZX  are  1e20,  i.e.    basically  no 
limits.
*MAT_RATE_SENSITIVE_COMPOSITE_FABRIC 
This is Material Type 158.  Depending on the type of failure surface, this model may be 
used  to  model  rate  sensitive  composite  materials  with  unidirectional  layers,  complete 
laminates,  and  woven  fabrics.    A  viscous  stress  tensor,  based  on  an  isotropic  Maxwell 
model with up to six terms in the Prony series expansion, is superimposed on the rate 
independent  stress  tensor  of  the  composite  fabric.    The  viscous  stress  tensor  approach 
should work reasonably well if the stress increases due to rate affects are up to 15% of 
the total stress.  This model is implemented for both shell and thick shell elements.  The 
viscous stress tensor is effective at eliminating spurious stress oscillations. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
EA 
F 
3 
4 
EB 
F 
4 
5 
6 
7 
8 
(EC) 
PRBA 
TAU1 
GAMMA1
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
GAB 
GBC 
GCA 
SLIMT1 
SLIMC1 
SLIMT2 
SLIMC2 
SLIMS 
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
F 
4 
Variable 
AOPT 
TSIZE 
ERODS 
SOFT 
Type 
F 
F 
F 
F 
  Card 4 
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
3 
ZP 
F 
4 
A1 
F 
F 
5 
FS 
F 
5 
A2 
F 
F 
6 
6 
A3 
F 
F 
7 
F 
8 
7 
8 
PRCA 
PRCB 
F
Card 5 
Variable 
1 
V1 
Type 
F 
  Card 6 
1 
2 
V2 
F 
2 
3 
V3 
F 
3 
4 
D1 
F 
4 
5 
D2 
F 
5 
6 
D3 
F 
6 
7 
8 
BETA 
F 
7 
8 
Variable 
E11C 
E11T 
E22C 
E22T 
GMS 
Type 
F 
F 
F 
F 
F 
2 
XT 
F 
2 
3 
YC 
F 
3 
4 
YT 
F 
4 
5 
SC 
F 
5 
6 
7 
8 
6 
7 
8 
  Card 7 
Variable 
1 
XC 
Type 
F 
  Card 8 
Variable 
Type 
1 
K 
F 
Viscoelastic  Cards.    Up  to  6  cards  may  be  input.    A  keyword  card  (with  a  “*”  in 
column 1) terminates this input if less than 6 cards are used.   
 Optional 
Variable 
Type 
1 
GI 
F 
2 
3 
4 
5 
6 
7 
8 
BETAI
*MAT_RATE_SENSITIVE_COMPOSITE_FABRIC 
DESCRIPTION
MID 
RO 
EA 
EB 
(EC) 
PRBA 
PRCA 
PRCB 
TAU1 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Ea, Young’s modulus - longitudinal direction 
Eb, Young’s modulus - transverse direction 
Ec, Young’s modulus - normal direction (not used) 
ba, Poisson’s ratio ba 
ca,  Poisson’s  ratio  ca,  can  be  defined  in  card  4,  col.    7,
default = PRBA 
cb,  Poisson’s  ratio  cb,  can  be  defined  in  card  4,  col.    8,
default = PRBA 
τ1, stress limit of the first slightly nonlinear part of the shear stress 
versus shear strain curve.  The values τ1 and γ1 are used to define 
a curve of shear stress versus shear strain.  These values are input
if FS, defined below, is set to a value of -1. 
GAMMA1 
γ1, strain limit of the first slightly nonlinear part of the shear stress
versus shear strain curve. 
GAB 
GBC 
GCA 
SLIMT1 
SLIMC1 
SLIMT2 
SLIMC2 
Gab, shear modulus ab 
Gbc, shear modulus bc 
Gca, shear modulus ca 
Factor  to  determine  the  minimum  stress  limit  after  stress
maximum (fiber tension). 
Factor  to  determine  the  minimum  stress  limit  after  stress
maximum (fiber compression). 
Factor  to  determine  the  minimum  stress  limit  after  stress
maximum (matrix tension). 
Factor  to  determine  the  minimum  stress  limit  after  stress
maximum (matrix compression).
VARIABLE   
DESCRIPTION
SLIMS 
AOPT 
Factor  to  determine  the  minimum  stress  limit  after  stress
maximum (shear). 
Material  axes  option  : 
EQ.0.0:  locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES,  and  then  rotated  about  the  shell  ele-
ment normal by the angle BETA. 
EQ.2.0:  globally orthotropic with material axes determined by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0:  locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by 
an angle (BETA) from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the
element normal. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
TSIZE 
Time step for automatic element deletion. 
ERODS 
Maximum  effective  strain  for  element  layer  failure.    A  value  of
unity would equal 100% strain. 
SOFT 
Softening reduction factor for strength in the crashfront. 
FS 
Failure surface type: 
EQ.1.0:  smooth  failure  surface  with  a  quadratic  criterion  for
both  the  fiber  (a)  and  transverse  (b)  directions.    This
option  can  be  used  with  complete  laminates  and  fab-
rics. 
EQ.0.0:  smooth  failure  surface  in  the  transverse  (b)  direction
with  a  limiting  value  in  the  fiber  (a)  direction.    This
model  is  appropriate  for  unidirectional  (UD)  layered
composites only. 
EQ.-1:  faceted  failure  surface.    When  the  strength  values  are 
reached then damage evolves in tension and compres-
*MAT_RATE_SENSITIVE_COMPOSITE_FABRIC 
DESCRIPTION
sion for both the fiber and transverse direction.  Shear
behavior  is  also  considered.    This  option  can  be  used
with complete laminates and fabrics. 
XP, YP, ZP 
Define coordinates of point p for AOPT = 1. 
A1, A2, A3 
Define components of vector a for AOPT = 2. 
V1, V2, V3 
Define components of vector v for AOPT = 3. 
D1, D2, D3 
Define components of vector d for AOPT = 2. 
BETA 
E11C 
E11T 
E22C 
E22T 
GMS 
XC 
XT 
YC 
YT 
SC 
K 
GI 
Material angle in degrees for AOPT = 0 and 3, may be overridden 
on the element card, see *ELEMENT_SHELL_BETA. 
Strain at longitudinal compressive strength, a-axis. 
Strain at longitudinal tensile strength, a-axis. 
Strain at transverse compressive strength, b-axis. 
Strain at transverse tensile strength, b-axis. 
Strain at shear strength, ab plane. 
Longitudinal compressive strength 
Longitudinal tensile strength, see below. 
Transverse compressive strength, b-axis, see below. 
Transverse tensile strength, b-axis, see below. 
Shear strength, ab plane. 
Optional bulk modulus for the viscoelastic material.  If nonzero a
Kelvin type behavior will be obtained.  Generally, K is set to zero.
Optional shear relaxation modulus for the ith term 
BETAI 
Optional shear decay constant for the ith term 
Remarks: 
See  the  remark  for  material  type  58,  *MAT_LAMINATED_COMPOSITE_FABRIC,  for 
the treatment of the composite material.
Rate effects are taken into account through a Maxwell model using linear viscoelasticity 
by a convolution integral of the form: 
𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)
∂𝜀𝑘𝑙
∂𝜏
𝑑𝜏
where 𝑔𝑖𝑗𝑘𝑙(𝑡−𝜏) is the relaxation functions for the different stress measures.  This stress is 
added to the stress tensor determined from the strain energy functional.  Since we wish 
to  include  only  simple  rate  effects,  the  relaxation  function  is  represented  by  six  terms 
from the Prony series: 
𝑔(𝑡) = ∑ 𝐺𝑚𝑒−𝛽𝑚𝑡
𝑚=1
We characterize this in the input by the shear moduli, 𝐺𝑖, and decay constants, 𝛽𝑖.  An 
arbitrary number of terms, not exceeding 6, may be used when applying the viscoelastic 
model.    The  composite  failure  is  not  directly  affected  by  the  presence  of  the  viscous 
stress tensor.
*MAT_CSCM 
This  is  material  type  159.    This  is  a  smooth  or  continuous  surface  cap  model  and  is 
available for solid elements in LS-DYNA.  The user has the option of inputting his own 
material  properties  (<BLANK>  option),  or  requesting  default  material  properties  for 
normal strength concrete (CONCRETE). 
Available options include: 
<BLANK> 
CONCRETE 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
RO 
NPLOT 
INCRE 
IRATE 
ERODE 
RECOV 
ITRETRC 
F 
2 
I 
3 
F 
4 
I 
5 
F 
6 
F 
7 
I 
8 
Type 
A8 
  Card 2 
1 
Variable 
PRED 
Type 
F 
Card 3 for CONCRETE keyword option. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FPC 
DAGG 
UNITS 
Type 
F 
F
The remaining cards are read when the keyword option is left blank.  They are not read 
in when CONCRETE keyword option is active.  
  Card 3 
Variable 
Type 
1 
G 
F 
  Card 4 
1 
2 
K 
F 
2 
3 
4 
5 
6 
ALPHA 
THETA 
LAMDA 
BETA 
F 
3 
F 
4 
F 
5 
F 
6 
7 
NH 
F 
7 
8 
CH 
F 
8 
Variable 
ALPHA1 
THETA1 
LAMDA1 
BETA1 
ALPHA2 
THETA2 
LAMDA2 
BETA2 
Type 
F 
F 
  Card 5 
Variable 
Type 
  Card 6 
Variable 
Type 
1 
R 
F 
1 
B 
F 
  Card 7 
1 
2 
X0 
F 
2 
GFC 
F 
2 
F 
3 
W 
F 
3 
D 
F 
3 
Variable 
ETA0C 
NC 
ETA0T 
Type 
F 
F 
F 
F 
F 
4 
D1 
F 
4 
5 
D2 
F 
5 
F 
6 
F 
7 
F 
8 
6 
7 
8 
GFT 
GFS 
PWRC 
PWRT 
PMOD 
F 
4 
NT 
F 
F 
5 
F 
6 
F 
7 
F 
8 
OVERC 
OVERT 
SRATE 
REPOW 
F 
F 
F
MID 
*MAT_CSCM 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density. 
NPLOT 
Controls  what  is  written  as  component  7  to  the  d3plot  database.
LS-Prepost  always  blindly  labels  this  component  as  effective
plastic strain: 
EQ.1:  Maximum of brittle and ductile damage (default). 
EQ.2:  Maximum  of  brittle  and  ductile  damage,  with  recovery
of brittle damage. 
EQ.3:  Brittle damage. 
EQ.4:  Ductile damage. 
EQ.5:  κ  (intersection of cap with shear surface). 
EQ.6:  X0 (intersection of cap with pressure axis). 
EQ.7:  𝜀v
p (plastic volume strain). 
INCRE 
Maximum strain increment for subincrementation.  If left blank, a
default  value  is  set  during  initialization  based  upon  the  shear
strength and stiffness. 
IRATE 
Rate effects options: 
EQ.0:  Rate effects model turned off (default). 
EQ.1:  Rate effects model turned on. 
ERODE 
Elements  erode  when  damage  exceeds  0.99  and  the  maximum
principal  strain  exceeds  ERODE-1.0. 
  For  erosion  that  is 
independent of strain, set ERODE equal to 1.0.   Erosion does not
occur if ERODE is less than 1.0.
RECOV 
*MAT_159 
DESCRIPTION
The modulus is recovered in compression when RECOV is equal 
to  0  (default).    The  modulus  remains  at  the  brittle  damage  level
when  RECOV  is  equal  to  1.    Partial  recovery  is  modeled  for
values of RECOV between 0 and 1.  Two options are available: 
EQ.1:  Input a value between 0 and 1.  Recovery is based upon 
the sign of the pressure invariant only. 
EQ.2:  Input  a  value  between  10  and  11.    Recovery  is  based
upon the sign of both the pressure and volumetric strain.
In  this  case,  RECOV = RECOV-10,  and  a  flag  is  set  to 
request the volumetric strain check. 
IRETRC 
Cap retraction option: 
EQ.0:  Cap does not retract (default). 
EQ.1:  Cap retracts. 
PRED 
Pre-existing  damage  (0  ≤  PreD < 1).    If  left  blank,  the  default  is 
zero (no pre-existing damage). 
Define for the CONCRETE option only: 
  VARIABLE   
FPC 
DESCRIPTION
Unconfined  compression  strength,  f  'C.    Material  parameters  are 
internally  fit  to  data  for  unconfined  compression  strengths
between about 20 and 58 Mpa (2,901 to 8,412 psi), with emphasis
on the midrange between 28 and 48 MPa (4,061 and 6,962 psi).  If
left blank, default for FPC is 30 MPa. 
DAGG 
Maximum  aggregate  size,  Dagg.    Softening  is  fit  to  data  for
aggregate sizes between 8 and 32 mm (0.3 and 1.3 inches).  If left
blank, default for DAGG is 19 mm (3/4 inch). 
UNITS 
Units options: 
EQ.0:  GPa, mm, msec, Kg/mm3, kN 
EQ.1:  MPa, mm, msec, g/mm3, N 
EQ.2:  MPa, mm, sec, Mg/mm3, N 
EQ.3:  Psi, inch, sec, lbf-s2/inch4, lbf 
EQ.4:  Pa, m, sec, kg/m3, N
*MAT_CSCM 
  VARIABLE   
DESCRIPTION
G 
K 
ALPHA 
THETA 
Shear modulus. 
Bulk modulus. 
Tri-axial compression surface constant term, α. 
Tri-axial compression surface linear term, θ. 
LAMDA 
Tri-axial compression surface nonlinear term, λ. 
BETA 
Tri-axial compression surface exponent, β. 
ALPHA1 
Torsion surface constant term, α1. 
THETA1 
Torsion surface linear term, θ1. 
LAMDA1 
Torsion surface nonlinear term, λ1. 
BETA1 
Torsion surface exponent, β1. 
ALPHA2 
Tri-axial extension surface constant term, α2. 
THETA2 
Tri-axial extension surface linear term, θ2. 
LAMDA2 
Tri-axial extension surface nonlinear term, λ2. 
BETA2 
Tri-axial extension surface exponent, β2. 
NH 
CH 
R 
X0 
W 
D1 
D2 
B 
Hardening initiation, NH. 
Hardening rate, CH. 
Cap aspect ratio, R. 
Cap initial location, X0. 
Maximum plastic volume compaction, W. 
Linear shape parameter, D1. 
Quadratic shape parameter, D2. 
Ductile shape softening parameter, B.
VARIABLE   
GFC 
D 
GFT 
GFS 
PWRC 
PWRT 
DESCRIPTION
Fracture energy in uniaxial stress Gfc. 
Brittle shape softening parameter, D. 
Fracture energy in uniaxial tension, Gft. 
Fracture energy in pure shear stress, Gfs. 
Shear-to-compression transition parameter. 
Shear-to-tension transition parameter. 
PMOD 
Modify moderate pressure softening parameter. 
ETA0C 
Rate effects parameter for uniaxial compressive stress, η0c. 
NC 
Rate effects power for uniaxial compressive stress, NC. 
ETA0T 
Rate effects parameter for uniaxial tensile stress, η0t. 
NT 
Rate effects power for uniaxial tensile stress,  Nt. 
OVERC 
Maximum overstress allowed in compression. 
OVERT 
Maximum overstress allowed in tension. 
SRATE 
Ratio of effective shear stress to tensile stress fluidity parameters.
REPOW 
Power which increases fracture energy with rate effects. 
Model Formulation and Input Parameters:
Shear Surface
Smooth Intersection
Cap
Pressure
Figure  M159-1.    General  shape  of  concrete  model  yield  surface  in  two
dimensions. 
This  is  a  cap  model  with  a  smooth  intersection  between  the  shear  yield  surface  and 
hardening cap, as shown in Figure M159-1.   The initial damage surface coincides with 
the  yield  surface.    Rate  effects  are  modeled  with  viscoplasticity.    For  a  complete 
theoretical  description,  with  references  and  example  problems  see  [Murray  2007]  and 
[Murray, Abu-Odeh and Bligh 2007]. 
Stress Invariants. The yield surface is formulated in terms of three stress invariants:  𝐽1 is 
′  is the second invariant of the deviatoric stress 
the first invariant of the stress tensor, 𝐽2
′   is  the  third  invariant  of  the  deviatoric  stress  tensor.    The  invariants  are 
tensor,  and  𝐽3
defined in terms of the deviatoric stress tensor, Sij and pressure, P, as follows: 
𝐽1 = 3P 
′ =
𝐽2
′ =
𝐽3
SijSij 
SijSjkSki 
Plasticity Surface.  The three invariant yield function is based on these three invariants, 
and the cap hardening parameter, κ, as follows: 
′ , 𝜅) = 𝐽2
Here 𝐹f is the shear failure surface,  𝐹c is the hardening cap, and ℜ is the Rubin three-
invariant reduction factor.  The cap hardening parameter 𝜅  is the value of the pressure 
invariant at the intersection of the cap and shear surfaces. 
′ − ℜ2𝐹𝑓
𝑓 (𝐽1, 𝐽2
2𝐹𝑐 
′ , 𝐽3
Trial elastic stress invariants are temporarily updated via the trial elastic stress tensor, 
′𝑇.    Elastic  stress  states  are  modeled  when 
𝝈𝑇.    These  are  denoted  J1
′𝑇, 𝜅𝑇) ≤
𝑓 (𝐽1
′𝑇, 𝜅𝑇) ≤ 0.    Elastic-plastic  stress  states  are  modeled  when  𝑓 (𝐽1
′𝑇,  and  J3
𝑇,  J2
′𝑇, 𝐽3
′𝑇, 𝐽3
𝑇, 𝐽2
𝑇, 𝐽2
0.   In this case, the plasticity algorithm returns the stress state to the yield surface such 
′𝑃, 𝜅𝑃) = 0.    This  is  accomplished  by  enforcing  the  plastic  consistency 
that  𝑓 (𝐽1
condition with associated flow. 
′𝑃, 𝐽3
𝑃, 𝐽2
Shear  Failure  Surface.    The  strength  of  concrete  is  modeled  by  the  shear  surface  in  the 
tensile and low confining pressure regimes: 
𝐹𝑓 (J1) = 𝛼 − 𝜆 exp−𝛽 J1 + 𝜃𝐽1 
Here  the  values  of  𝛼, 𝛽, 𝜆, and 𝜃  are  selected  by  fitting  the  model  surface  to  strength 
measurements  from  triaxial  compression  (TXC)  tests  conducted  on  plain  concrete 
cylinders. 
′   (principal  stress 
Rubin  Scaling  Function.    Concrete  fails  at  lower  values  of  √3𝐽2
difference)  for  triaxial extension  (TXE)  and  torsion  (TOR)  tests  than  it  does  for  TXC  tests 
conducted at the same pressure.  The Rubin scaling function ℜ determines the strength 
of  concrete  for  any  state  of  stress  relative  to the  strength  for  TXC,  via ℜFf.    Strength  in 
torsion is modeled as Q1Ff .  Strength in TXE is modeled as Q2Ff, where:  
𝑄1 = 𝛼1 − 𝜆1exp−𝛽1J1 + 𝜃1𝐽1 
𝑄2 = 𝛼2 − 𝜆2exp−𝛽2J1 + 𝜃2𝐽1 
Cap Hardening Surface. The strength of concrete is modeled by a combination of the cap 
and  shear  surfaces  in  the  low  to  high  confining  pressure  regimes.    The  cap  is  used  to 
model  plastic  volume  change  related  to  pore  collapse  (although  the  pores  are  not 
explicitly  modeled).      The  isotropic  hardening  cap  is  a  two-part  function  that  is  either 
unity or an ellipse: 
𝐹𝑐( 𝐽1, 𝜅 ) = 1 −
[𝐽1 − 𝐿 (𝜅)][ |𝐽1 − 𝐿(𝜅)| + 𝐽1 − 𝐿(𝜅) ]
2  [𝑋(𝜅) − 𝐿 (𝜅)] 2
where 𝐿(𝜅) is defined as: 
𝐿(𝜅) = {
if    𝜅 > 𝜅0
𝜅0 otherwise
The equation for 𝐹𝑐 is equal to unity for 𝐽1 ≤ 𝐿(𝜅).  It describes the ellipse for J1 > L(κ).  
The intersection of the shear surface and the cap is at J1 = κ.  κ0 is the value of J1 at the 
initial intersection of the cap and shear surfaces before hardening is engaged (before the 
cap  moves).    The  equation  for  L(κ)  restrains  the  cap  from  retracting  past  its  initial 
location at κ0. 
The  intersection  of  the  cap  with  the  J1  axis  is  at  J1 = X(κ).    This  intersection  depends 
upon the cap ellipticity ratio R, where R is the ratio of its major to minor axes: 
𝑋(𝜅) = 𝐿(𝜅) + R𝐹𝑓 [𝐿(𝜅)]
The  cap  expands  (X(κ) 
The  cap  moves  to  simulate  plastic  volume  change. 
and κ increase)  to  simulate  plastic  volume  compaction.    The  cap  contracts  (X(κ)  and κ 
decrease) to simulate plastic volume expansion, called dilation.   The motion (expansion 
and contraction) of the cap is based upon the hardening rule: 
𝑝 = 𝑊[1 − 𝑒−𝐷1(𝑋−𝑋0)−𝐷2(𝑋−𝑋0)2
𝜀𝑣
] 
p the plastic volume strain, W is the maximum plastic volume strain, and D1 and 
Here 𝜀v
D2 are model input parameters.  X0 is the initial location of the cap when κ = κ0. 
The five input parameters (X0, W, D1, D2, and R) are obtained from fits to the pressure-
volumetric strain curves in isotropic compression and uniaxial strain. X0 determines the 
pressure at which compaction initiates in isotropic compression. R, combined with X0, 
determines  the  pressure  at  which  compaction  initiates  in  uniaxial  strain.  D1,  and  D2 
determine  the  shape  of  the  pressure-volumetric  strain  curves.    W  determines  the 
maximum plastic volume compaction. 
Shear  Hardening  Surface.    In  unconfined  compression,  the  stress-strain  behavior  of 
concrete  exhibits  nonlinearity  and  dilation  prior  to  the  peak.        Such  behavior  is  be 
modeled with an initial shear yield surface, NHFf , which hardens until it coincides with 
the  ultimate  shear  yield  surface,  Ff.    Two  input  parameters  are  required.    One 
parameter, NH, initiates hardening by setting the location of the initial yield surface.  A 
second parameter, CH, determines the rate of hardening (amount of nonlinearity). 
Damage.  Concrete  exhibits  softening  in  the  tensile  and  low  to  moderate  compressive 
regimes. 
d = (1 − 𝑑)𝜎ij
𝜎ij
vp 
A  scalar  damage  parameter,  d,  transforms  the  viscoplastic  stress  tensor  without 
damage,  denoted  σvp,  into  the  stress  tensor  with  damage,  denoted  σd.    Damage 
accumulation  is  based  upon  two  distinct  formulations,  which  we  call  brittle  damage 
and ductile damage.  The initial damage threshold is coincident with the shear plasticity 
surface, so the threshold does not have to be specified by the user. 
Ductile Damage.   Ductile damage accumulates when the pressure (P) is compressive and 
an  energy-type  term,  τc,  exceeds  the  damage  threshold,  τ0c. 
  Ductile  damage 
accumulation depends upon the total strain components, εij, as follows: 
The  stress  components  σij  are  the  elasto-plastic  stresses  (with  kinematic  hardening) 
calculated before application of damage and rate effects. 
𝜏c =   √
𝜎𝑖𝑗𝜀𝑖𝑗
Brittle Damage.  Brittle damage accumulates when the pressure is tensile and an energy-
type term, τt, exceeds the damage threshold, τ0t.    Brittle damage accumulation depends 
upon the maximum principal strain, ε max, as follows: 
Softening Function. As damage accumulates, the damage parameter d increases from an 
initial value of zero, towards a maximum value of one, via the following formulations: 
𝜏t = √𝐸 𝜀 max
Brittle Damage: 𝑑(𝜏𝑡) =  
Ductile Damage:
𝑑(𝜏𝑐) =  
0.999
𝑑max
1 + 𝐷
 [
1 + 𝐷 𝑒−𝐶(𝜏𝑡−𝜏0𝑡) − 1]
1 + 𝐵𝑒−𝐴(𝜏𝑐−𝜏0𝑐) − 1]
1 + 𝐵
 [
The  damage  parameter  that  is  applied  to  the  six  stresses  is  equal  to  the  current 
maximum of the brittle or ductile damage parameter.  The parameters A and B or C and 
D  set  the  shape  of  the  softening  curve  plotted  as  stress-displacement  or  stress-strain.   
The parameter dmax is the maximum damage level that can be attained.  It is calculated 
internally  calculated  and  is  less  than  one  at  moderate  confining  pressures.    The 
compressive softening parameter, A, may also be reduced with confinement, using the 
input parameter pmod, as follows: 
𝐴 = 𝐴(𝑑max + 0.001)pmod 
Regulating  Mesh  Size  Sensitivity.      The  concrete  model  maintains  constant  fracture 
energy,  regardless  of  element  size.    The  fracture  energy  is  defined  here  as  the  area 
under the stress-displacement curve from peak strength to zero strength.  This is done 
by  internally  formulating  the  softening  parameters  A  and  C  in  terms  of  the  element 
length,  l  (cube  root  of  the  element  volume),  the  fracture  energy,  Gf,  the  initial  damage 
threshold, τ0t or τ0c, and the softening shape parameters, D or B. 
The fracture energy is calculated from up to five user-specified input parameters: GFC, 
GFS, GFT, PWRC, and PWRT.  The user specifies three distinct fracture energy values.  
These are the fracture energy in uniaxial tensile stress, GFT, pure shear stress, GFS, and 
uniaxial compressive stress, GFC.  The model internally selects the fracture energy from 
equations  which  interpolate  between  the  three  fracture  energy  values  as  a  function  of 
the  stress  state  (expressed  via  two  stress  invariants).    The  interpolation  equations 
depend upon the user-specified input powers PWRC and PWRT, as follows.
Tensile Pressure: 𝐺𝑓 = GFS +
Compressive Pressure: 𝐺𝑓 = GFS +
𝑘𝑡
⏞⏞⏞⏞⏞⏞⏞
PWRT
⎜⎜⎜⎛ −𝐽1
⎟⎟⎟⎞
′
√3𝐽2
⎠
⎝
𝑘𝑐
⏞⏞⏞⏞⏞⏞⏞
PWRC
⎜⎜⎜⎛ 𝐽1
⎟⎟⎟⎞
′
√3𝐽2
⎠
⎝
[GFT − GFS]
[GFC − GFS]
The internal parameters 𝑘𝑐 and 𝑘𝑡 are restricted to the interval [0,1]. 
Element  Erosion.    An  element  losses  all  strength  and  stiffness  as  d→1.    To  prevent 
computational difficulties with very low stiffness, element erosion is available as a user 
option.  An element erodes when d > 0.99 and the maximum principal strain is greater 
than a user supplied input value, ERODE-1.0. 
Viscoplastic  Rate  Effects.    At  each  time  step,  the  viscoplastic  algorithm  interpolates 
p,  to 
between  the  elastic  trial  stress,  𝜎𝑖j
set the viscoplastic stress (with rate effects), 𝜎𝑖j
T,  and  the  inviscid  stress  (without  rate  effects),  𝜎𝑖j
vp: 
vp = (1 − 𝛾)σij
σij
p 
T + 𝛾σij
where, 
𝛾 =
Δt/𝜂
1 + Δt/𝜂
. 
This interpolation depends upon the effective fluidity coefficient, η, and the time step, 
Δt.    The  effective  fluidity  coefficient  is  internally  calculated  from  five  user-supplied 
input parameters and interpolation equations: 
Tensile Pressure: 𝜂 = 𝜂𝑠   +
Compressive Pressure:
𝜂 = 𝜂𝑠 +
where, 
PWRT
⎟⎟⎟⎞
⎠
PWRC
⎜⎜⎜⎛ −𝐽1
′
√3𝐽2
⎝
⎜⎜⎜⎛ 𝐽1
′
√3𝐽2
⎝
⎟⎟⎟⎞
⎠
[𝜂𝑡 − 𝜂𝑠]
[𝜂𝑐 − 𝜂𝑠]
𝜂𝑠 = SRATE × 𝜂𝑡 
𝜂𝑡 =
ETA0T
𝜖 ̇NT  
𝜂𝑐 =
ETA0C
𝜖 ̇NC
The input parameters are ΕΤΑ0Τ  and NT for fitting uniaxial tensile stress data, ΕΤΑ0Χ 
and  NC  for  fitting  the  uniaxial  compressive  stress  data,  and  SRATE  for  fitting  shear 
stress data.  The effective strain rate is 𝜀̇. 
This viscoplastic model may predict substantial rate effects at high strain rates (𝜀̇ > 100).  
To limit rate effects at high strain rates, the user may input overstress limits in tension 
OVERT  and  compression  OVERC.    These  input  parameters  limit  calculation  of  the 
fluidity parameter, as follows: 
if 𝐸𝜖 ̇𝜂 > OVER,  then 𝜂 =
𝐸𝜖 ̇
where m = OVERT when the pressure is tensile, and m = OVERC when the pressure is 
compressive. 
The user has the option of increasing the fracture energy as a function of effective strain 
rate via the REPOW input parameter, as follows: 
Gf
rate = Gf (1 +
Eε̇η
f′
rate  is  the  fracture  energy  enhanced  by  rate  effects,  and  f′  is  the  yield  strength 
Here  Gf
before application of rate effects (which is calculated internally by the model).  The term 
in brackets is greater than, or equal to one, and is the approximate ratio of the dynamic 
to static strength.
)
REPOW
*MAT_ALE_INCOMPRESSIBLE 
This is Material Type 160.  This card allows to solve incompressible flows with the ALE 
solver.  It should be used with the element formulation 6 and 12 in *SECTION_SOLID 
(elform = 6 or 12).  A projection method enforces the incompressibility condition. 
5 
6 
7 
8 
  Card 1 
1 
Variable 
MID 
Type 
I 
2 
RO 
F 
3 
PC 
F 
4 
MU 
F 
Default 
none 
none 
0.0 
0.0 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TOL 
DTOUT 
NCG 
METH 
Type 
F 
F 
I 
I 
Default 
1e-8 
1e10 
50 
-7 
  VARIABLE   
DESCRIPTION
MID 
RO 
PC 
MU 
TOL 
Material ID.  A unique number or label not exceeding 8 charaters
must  be  specified.    Material  ID  is  referenced  in  the  *PART  card
and must be unique 
Material density 
Pressure cutoff (< or = 0.0) 
Dynamic viscosity coefficient 
Tolerance for the convergence of the conjugate gradient 
DTOUT 
Time interval between screen outputs 
NCG 
Maximum number of  loops in the conjugate gradient
VARIABLE   
DESCRIPTION
METH 
Conjugate gradient methods: 
EQ.-6:  solves the poisson equation for the pressure 
EQ.-7:  solves the poisson equation for the pressure increment
*MAT_COMPOSITE_MSC_{OPTION} 
Available options include: 
<BLANK> 
DMG 
These  are  Material  Types  161  and  162.    These  models  may  be  used  to  model  the 
progressive  failure  analysis  for  composite  materials  consisting  of  unidirectional  and 
woven  fabric  layers.    The  progressive  layer  failure  criteria  have  been  established  by 
adopting the methodology developed by Hashin [1980] with a generalization to include 
the effect of highly constrained pressure on composite failure.  These failure models can 
be used to effectively simulate fiber failure, matrix damage, and delamination behavior 
under all conditions - opening, closure, and sliding of failure surfaces.  The model with 
DMG  option  (material  162)  is  a  generalization  of  the  basic  layer  failure  model  of 
Material  161  by  adopting  the  damage  mechanics  approach  for  characterizing  the 
softening behavior after damage initiation.  These models require an additional license 
from Materials Sciences Corporation, which developed and supports these models. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
EA 
F 
3 
4 
EB 
F 
4 
5 
EC 
F 
5 
Variable 
GAB 
GBC 
GCA 
AOPT 
MACF 
Type 
F 
F 
F 
F 
I 
  Card 3 
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
3 
ZP 
F 
4 
A1 
F 
5 
A2 
F 
6 
7 
8 
PRBA 
PRCA 
PRCB 
F 
7 
F 
8 
7 
8 
F 
6 
6 
A3
Card 4 
Variable 
1 
V1 
Type 
F 
  Card 5 
1 
2 
V2 
F 
2 
3 
V3 
F 
3 
4 
D1 
F 
4 
5 
D2 
F 
5 
6 
D3 
F 
6 
7 
8 
BETA 
F 
7 
8 
Variable 
SAT 
SAC 
SBT 
SBC 
SCT 
SFC 
SFS 
SAB 
Type 
F 
  Card 6 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
Variable 
SBC 
SCA 
SFFC 
AMODEL 
PHIC 
E_LIMT 
S_DELM 
Type 
F 
  Card 7 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
8 
Variable 
OMGMX 
ECRSH 
EEXPN 
CERATE1
AM1 
Type 
F 
F 
F 
F 
F 
Failure Card.  Additional card for DMG keyword option. 
  Card 8 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
AM2 
AM3 
AM4 
CERATE2 CERATE3 CERATE4 
Type 
F 
F 
F 
F 
F 
F 
  VARIABLE   
MID 
LS-DYNA R10.0 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
RO 
EA 
EB 
EC 
PRBA 
PRCA 
PRCB 
GAB 
GBC 
GCA 
Mass density 
Ea, Young’s modulus - longitudinal direction 
Eb, Young’s modulus - transverse direction 
Ec, Young’s modulus - through thickness direction 
ba, Poisson’s ratio ba 
ca, Poisson’s ratio ca 
cb, Poisson’s ratio cb 
Gab, shear modulus ab 
Gbc, shear modulus bc 
Gca, shear modulus ca 
AOPT 
Material axes option, see Figure 2.1: 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes as shown in Figure 2.1.  Nodes 1, 2, and
4 of an element are identical to the Nodes used for the
definition of a  coordinate system by *DEFINE_COOR-
DINATE_NODES. 
EQ.1.0: locally orthotropic with material axes determined by a 
point  in  space  and  the  global  location  of  the  element
center, to define the a-direction. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the
element  normal.    The  plane  of  a  solid  element  is  the 
midsurface between the inner surface and outer surface
defined by the first four nodes and the last four nodes
of the connectivity of the element, respectively. 
EQ.4.0: locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector  v,  and 
an originating point, p, which define the centerline ax-
is.  This option is for solid elements only. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
MACF 
Material axes change flag: 
EQ.1: No change, default, 
EQ.2: switch material axes a and b, 
EQ.3: switch material axes a and c, 
EQ.4: switch material axes b and c. 
XP, YP, ZP 
Define coordinates of point p for AOPT = 1 and 4. 
A1, A2, A3 
Define components of vector a for AOPT = 2. 
V1, V2, V3 
Define components of vector v for AOPT = 3 and 4. 
D1, D2, D3 
Define components of vector d for AOPT = 2. 
BETA 
Layer in-plane rotational angle in degrees. 
SAT 
SAC 
SBT 
SBC 
SCT 
SFC 
SFS 
SAB 
SBC 
SCA 
Longitudinal tensile strength 
Longitudinal compressive strength 
Transverse tensile strength 
Transverse compressive strength 
Through thickness tensile strength 
Crush strength 
Fiber mode shear strength 
Matrix mode shear strength, ab plane, see below. 
Matrix mode shear strength, bc plane, see below. 
Matrix mode shear strength, ca plane, see below. 
SFFC 
Scale factor for residual compressive strength
AMODEL 
Material models: 
EQ.1.0: Unidirectional layer model 
EQ.2.0: Fabric layer model 
PHIC 
Coulomb friction angle for matrix and delamination failure, < 90 
E_LIMT 
Element eroding axial strain 
S_DELM 
Scale factor for delamination criterion 
OMGMX 
Limit damage parameter for elastic modulus reduction 
ECRSH 
Limit compressive volume strain for element eroding 
EEXPN 
Limit tensile volume strain for element eroding 
CERATE1 
Coefficient for strain rate dependent strength properties 
AM1 
AM2 
AM3 
AM4 
Coefficient for strain rate softening property for fiber damage in a 
direction. 
Coefficient for strain rate softening property for fiber damage in b
direction. 
Coefficient  for  strain  rate  softening  property  for  fiber  crush  and
punch shear damage. 
Coefficient  for  strain  rate  softening  property  for  matrix  and 
delamination damage. 
CERATE2 
Coefficient for strain rate dependent axial moduli. 
CERATE3 
Coefficient for strain rate dependent shear moduli. 
CERATE4 
Coefficient for strain rate dependent transverse moduli. 
Material Models: 
in 
The  unidirectional  and  fabric  layer  failure  criteria  and  the  associated  property 
degradation models for material 161 are described as follows.  All the failure criteria are 
expressed 
stresses 
(𝜎𝑎, 𝜎𝑏, 𝜎𝑐, 𝜏𝑎𝑏, 𝜏𝑏𝑐, 𝜏𝑐𝑎)  and  the  associated  elastic  moduli  are  (𝐸𝑎, 𝐸𝑏, 𝐸𝑐, 𝐺𝑎𝑏, 𝐺𝑏𝑐, 𝐺𝑐𝑎).  
Note that for the unidirectional model, a, b and c denote the fiber, in-plane transverse 
and out-of-plane directions, respectively, while for the fabric model, a, b and  c denote 
the in-plane fill, in-plane warp and out-of-plane directions, respectively. 
components  based  on  ply 
terms  of 
stress 
level
Unidirectional lamina model: 
Three  criteria  are  used  for  fiber  failure,  one  in  tension/shear,  one  in  compression  and 
another  one  in  crush  under  pressure.    They  are  chosen  in  terms  of  quadratic  stress 
forms as follows: 
Tensile/shear fiber mode: 
𝑓1 = (
)
〈𝜎𝑎〉
𝑆𝑎𝑇
+ (
2 + 𝜏𝑐𝑎
𝜏𝑎𝑏
𝑆𝐹𝑆
) − 1 = 0 
Compression fiber mode: 
Crush mode: 
𝑓2 = (
)
′〉
〈𝜎𝑎
𝑆𝑎𝐶
− 1 = 0,
𝜎𝑎
′ = −𝜎𝑎 + ⟨−
𝜎𝑏 + 𝜎𝑐
⟩ 
𝑓3 = (
⟨𝑝⟩
𝑆𝐹𝐶
)
− 1 = 0,
𝑝 = −
𝜎𝑎 + 𝜎𝑏 + 𝜎𝑐
⟩ are Macaulay brackets, 𝑆𝑎𝑇 and 𝑆𝑎𝐶 are the tensile and compressive strengths 
where ⟨
in the fiber direction, and 𝑆𝐹𝑆 and 𝑆𝐹𝐶 are the layer strengths associated with the fiber 
shear and crush failure, respectively. 
Matrix mode failures must occur without fiber failure, and hence they will be on planes 
parallel  to  fibers.    For  simplicity,  only  two  failure  planes  are  considered:  one  is 
perpendicular to the planes of layering and the other one is parallel to them.  The matrix 
failure  criteria  for  the  failure  plane  perpendicular  and  parallel  to  the  layering  planes, 
respectively, have the forms: 
Perpendicular matrix mode: 
𝑓4 = (
)
⟨𝜎𝑏⟩
𝑆𝑏𝑇
+ (
𝜏𝑏𝑐
′ )
𝑆𝑏𝑐
+ (
)
𝜏𝑎𝑏
𝑆𝑎𝑏
− 1 = 0 
Parallel matrix mode (Delamination): 
(
𝑓5 = 𝑆2
𝜏𝑏𝑐
"
𝑆𝑏𝑐
where SbT is the transverse tensile strength.  Based on the Coulomb-Mohr theory, the 
shear strengths for the transverse shear failure and the two axial shear failure modes are 
assumed to be the forms, 
⟨𝜎𝑐⟩
𝑆𝑏𝑇
− 1 = 0 
𝜏𝑐𝑎
𝑆𝑐𝑎
+ (
+ (
)
)
)
}⎫
⎭}⎬
{⎧
⎩{⎨
𝑆𝑎𝑏 = 𝑆𝑎𝑏
′ = 𝑆𝑏𝑐
𝑆𝑏𝑐
𝑆𝑐𝑎 = 𝑆𝑐𝑎
(0) + tan(𝜑)⟨−𝜎𝑏⟩ 
(0) + tan(𝜑)⟨−𝜎𝑏⟩ 
(0) + tan(𝜑)⟨−𝜎𝑐⟩
" = 𝑆𝑏𝑐
𝑆𝑏𝑐
(0) + tan(𝜑)⟨−𝜎𝑐⟩ 
where ϕ is a material constant as tan(𝜑) is similar to the coefficient of friction, and 𝑆𝑎𝑏
(0)are the shear strength values of the corresponding tensile modes. 
(0)and 𝑆𝑏𝑐
𝑆𝑐𝑎
(0), 
Failure  predicted  by  the  criterion  of  f4  can  be  referred  to  as  transverse  matrix  failure, 
while the matrix failure predicted by f5, which is parallel to the layer, can be referred as 
the delamination mode when it occurs within the elements that are adjacent to the ply 
interface.    Note  that  a  scale  factor  S  is  introduced  to  provide  better  correlation  of 
delamination area with experiments.  The scale factor S can be determined by fitting the 
analytical prediction to experimental data for the delamination area. 
When fiber failure in tension/shear mode is predicted in a layer by f1, the load carrying 
capacity of that layer is completely eliminated.  All the stress components are reduced 
to zero instantaneously (100 time steps to avoid numerical instability).  For compressive 
fiber  failure,  the  layer  is  assumed  to  carry  a  residual  axial  load,  while  the  transverse 
load carrying capacity is reduced to zero.  When the fiber compressive failure mode is 
reached due to f2, the axial layer compressive strength stress is assumed to reduce to a 
residual value 𝑆𝑅𝐶 (=SFFC × 𝑆𝐴𝐶).  The axial stress is then assumed to remain constant, 
i.e.,  𝜎𝑎   =   −𝑆𝑅𝐶,  for  continuous  compressive  loading,  while  the  subsequent  unloading 
curve follows a reduced axial modulus to zero axial stress and strain state.  When the 
fiber crush failure occurs, the material is assumed to behave elastically for compressive 
pressure, p > 0, and to carry no load for tensile pressure, p < 0. 
(0)and  𝑆𝑏𝑐
When a matrix failure (delamination) in the a-b plane is predicted, the strength values 
(0)  are  set  to  zero.    This  results  in  reducing  the  stress  components  𝜎𝑐, 𝜏𝑏𝑐 
for  𝑆𝑐𝑎
and 𝜏𝑐𝑎 to the fractured material strength surface.  For tensile mode, 𝜎𝑐 > 0, these stress 
components are reduced to zero.  For compressive mode, 𝜎𝑐 < 0, the normal stress 𝜎𝑐 is 
assumed  to  deform  elastically  for  the  closed  matrix  crack.    Loading  on  the  failure 
envelop,  the  shear  stresses  are  assumed  to  ‘slide’  on  the  fractured  strength  surface 
(frictional  shear  stresses)  like  in  an  ideal  plastic  material,  while  the  subsequent 
unloading shear stress-strain path follows reduced shear moduli to the zero shear stress 
and strain state for both 𝜏𝑏𝑐 and 𝜏𝑐𝑎 components. 
(0)and  𝑆𝑏𝑐
The post failure behavior for the matrix crack in the a-c plane  due to f4 is  modeled in 
the same fashion as that in the a-b plane as described above.  In this case, when failure 
(0)are  reduced  to  zero  instantaneously.    The  post  fracture  response  is 
occurs,  𝑆𝑎𝑏
(0)=  0.    For  tensile  mode, 
then  governed  by  failure  criterion  of  f5  with  𝑆𝑎𝑏
𝜎𝑏 > 0,  𝜎𝑏,  𝜏𝑎𝑏  and  𝜏𝑏𝑐  are  zero.    For  compressive  mode,  𝜎𝑏 < 0,  𝜎𝑏  is  assumed  to  be 
elastic,  while  𝜏𝑎𝑏  and  𝜏𝑏𝑐  ‘slide’  on  the  fracture  strength  surface  as  in  an  ideal  plastic 
material, and the unloading path follows reduced shear moduli to the zero shear stress 
and  strain  state.    It  should  be  noted  that  𝜏𝑏𝑐  is  governed  by  both  the  failure  functions 
and should lie within or on each of these two strength surfaces. 
(0)=  0  and  𝑆𝑏𝑐
Fabric lamina model: 
The  fiber  failure  criteria  of  Hashin  for  a  unidirectional  layer  are  generalized  to 
characterize  the  fiber  damage  in  terms  of  strain  components  for  a  plain  weave  layer.  
The  fill  and  warp  fiber  tensile/shear  failure  are  given  by  the  quadratic  interaction 
between the associated axial and shear stresses, i.e. 
2   +   𝜏𝑐𝑎
2 )
𝑆𝑎𝐹𝑆
2 )
2   +   𝜏𝑏𝑐
𝑆𝑏𝐹𝑆
⟨𝜎𝑏⟩
𝑆𝑏𝑇
⟨𝜎𝑎⟩
𝑆𝑎𝑇
− 1 = 0 
− 1 = 0 
𝑓7   = (
𝑓6   = (
(𝜏𝑎𝑏
(𝜏𝑎𝑏
)
+
+
)
where  𝑆𝑎𝑇and  𝑆𝑏𝑇  are  the  axial  tensile  strengths  in  the  fill  and  warp  directions, 
respectively, and 𝑆𝑎𝐹𝑆 and 𝑆𝑏𝐹𝑆 are the layer shear strengths due to fiber shear failure in 
the fill and warp directions.  These failure criteria are applicable when the associated 𝜎𝑎 
or 𝜎𝑏 is positive.  It is assumed 𝑆𝑎𝐹𝑆= SFS, and 
𝑆𝑏𝐹𝑆   = SFS ×
𝑆𝑏𝑇
𝑆𝑎𝑇
. 
When 𝜎𝑎 or 𝜎𝑏is compressive, it is assumed that the in-plane compressive failure in both 
the fill and warp directions are given by the maximum stress criterion, i.e. 
𝑓8  =   [
′⟩
⟨𝜎𝑎
]
𝑆𝑎𝐶
𝑓9   =   [
]
′⟩
⟨𝜎𝑏
𝑆𝑏𝐶
  −  1  =  0,      𝜎𝑎
′   =   −𝜎𝑎   +   ⟨−𝜎𝑐⟩ 
  −  1  =  0,      𝜎𝑏
′   =    −𝜎𝑏   +   ⟨−𝜎𝑐⟩ 
where  𝑆𝑎𝐶and  𝑆𝑏𝐶  are  the  axial  compressive  strengths  in  the  fill  and  warp  directions, 
respectively.  The crush failure under compressive pressure is 
𝑓10   =   (
⟨𝑝⟩
𝑆𝐹𝐶
)
− 1 = 0,      𝑝 = −
𝜎𝑎 + 𝜎𝑏 + 𝜎𝑐  
A plain weave layer can fail under in-plane shear stress without the occurrence of fiber 
breakage.  This in-plane matrix failure mode is given by 
𝑓11 = (
𝜏𝑎𝑏
𝑆𝑎𝑏
)
− 1 = 0 
where 𝑆𝑎𝑏 is the layer shear strength due to matrix shear failure. 
Another failure mode, which is due to the quadratic interaction between the thickness 
stresses,  is  expected  to  be  mainly  a  matrix  failure.    This  through  the  thickness  matrix 
failure criterion is 
𝑓12   =   𝑆2 {(
⟨𝜎𝑐⟩
𝑆𝑐𝑇
)
2 
+ (
𝜏𝑏𝑐
𝑆𝑏𝑐
)
+ (
𝜏𝑐𝑎
𝑆𝑐𝑎
)
} − 1 = 0
where  𝑆𝑐𝑇  is  the  through  the  thickness  tensile  strength,  and  𝑆𝑏𝑐,  and  𝑆𝑐𝑎  are  the  shear 
strengths assumed to depend on the compressive normal stress 𝜎𝑐, i.e., 
𝑆𝑐𝑎
{
𝑆𝑏𝑐
} = {
(0)
𝑆𝑐𝑎
(0)} + tan(𝜑)⟨−𝜎𝑐⟩ 
𝑆𝑏𝑐
When failure predicted by this criterion occurs within elements that are adjacent to the 
ply  interface,  the  failure  plane  is  expected  to  be  parallel  to  the  layering  planes,  and, 
thus,  can  be  referred  to  as  the  delamination  mode.    Note  that  a  scale  factor  S  is 
introduced  to  provide  better  correlation  of  delamination  area  with  experiments.    The 
scale factor S can be determined by fitting the analytical prediction to experimental data 
for the delamination area. 
Similar  to  the  unidirectional  model,  when  fiber  tensile/shear  failure  is  predicted  in  a 
layer  by  f6  or  f7,  the  load  carrying  capacity  of  that  layer  in  the  associated  direction  is 
completely  eliminated.    For  compressive  fiber  failure  due  to  by  f8  or  f9,  the  layer  is 
assumed  to  carry  a  residual  axial  load  in  the  failed  direction,  while  the  load  carrying 
capacity  transverse  to  the  failed  direction  is  assumed  unchanged.    When  the 
compressive axial stress in a layer reaches the compressive axial strength 𝑆𝑎𝐶 or 𝑆𝑏𝐶, the 
axial layer stress is assumed to be reduced to the residual strength 𝑆𝑎𝑅𝐶 or 𝑆𝑏𝑅𝐶 where 
𝑆𝑎𝑅𝐶   =  SFFC × 𝑆𝑎𝐶  and  𝑆𝑏𝑅𝐶   =  SFFC × 𝑆𝑏𝐶.    The  axial  stress  is  assumed  to  remain 
constant,  i.e.,  𝜎𝑎   =   −𝑆𝑎𝐶𝑅  or  𝜎𝑏   =   −𝑆𝑏𝐶𝑅,  for  continuous  compressive  loading,  while 
the subsequent unloading curve follows a reduced axial modulus.  When the fiber crush 
failure  is  occurred,  the  material  is  assumed  to  behave  elastically  for  compressive 
pressure, p > 0, and to carry no load for tensile pressure, p < 0. 
When  the  in-plane  matrix  shear  failure  is  predicted  by  f11  the  axial  load  carrying 
capacity within a failed element is assumed unchanged, while the in-plane shear stress 
is assumed to be reduced to zero. 
For through the thickness matrix (delamination) failure given by equations f12, the in-
plane  load  carrying  capacity  within  the  element  is  assumed  to  be  elastic,  while  the 
(0),  are  set  to  zero.    For  tensile  mode, 
(0)  and  𝑆𝑏𝑐
strength  values  for  the  tensile  mode,  𝑆𝑐𝑎
𝜎𝑐 > 0,  the  through  the  thickness  stress  components  are  reduced  to  zero.    For 
compressive  mode, 𝜎𝑐 < 0,  𝜎𝑐  is  assumed  to  be  elastic,  while  𝜏𝑏𝑐  and  𝜏𝑐𝑎  ‘slide’  on  the 
fracture strength surface as in an ideal plastic material, and the unloading path follows 
reduced shear moduli to the zero shear stress and strain state. 
The  effect  of  strain-rate  on  the  layer  strength  values  of  the  fiber  failure  modes  is 
modeled by the strain-rate dependent functions for the strength values {𝑆𝑅𝑇} as 
{𝑆𝑅𝑇 } = {𝑆0 } ( 1 + 𝐶rate1 ln
̇}
{𝜀̅
𝜀̇0
)
{𝑆𝑅𝑇} =
⎧𝑆𝑎𝑇
⎫
}
{
}
𝑆𝑎𝐶
{
}
{
}
{
𝑆𝑏𝑇
⎬
⎨
𝑆𝑏𝐶
}
{
}
{
𝑆𝐹𝐶
}
{
}
{
𝑆𝐹𝑆 ⎭
⎩
,
{𝜀̅
̇} =
⎧
{{{{{
{{{{{
⎨
⎩
∣𝜀̇𝑎∣
∣𝜀̇𝑎∣
∣𝜀̇𝑏∣
∣𝜀̇𝑏∣
∣𝜀̇𝑐∣
2 )
2 + 𝜀̇𝑏𝑐
(𝜀̇𝑐𝑎
1/2
⎫
}}}}}
}}}}}
⎬
⎭
where Crate is the strain-rate constants, and {𝑆0 }are the strength values of {𝑆𝑅𝑇 } at the 
reference strain-rate 𝜀̇0. 
Damage model: 
The  damage  model  is  a  generalization  of  the  layer  failure  model  of  Material  161  by 
adopting  the  MLT  damage  mechanics  approach,  Matzenmiller  et  al.    [1995],  for 
characterizing  the  softening  behavior  after  damage  initiation.    Complete  model 
description is given in Yen [2002].  The damage functions, which are expressed in terms 
of  ply  level  engineering  strains,  are  converted  from  the  above  failure  criteria  of  fiber 
and matrix failure modes by neglecting the Poisson’s effect.  Elastic moduli reduction is 
expressed in terms of the associated damage parameters 𝜛𝑖: 
′ = (1 − 𝜛𝑖)𝐸𝑖 
𝐸𝑖
𝜛𝑖 = 1 − exp (−
𝑚𝑖
𝑟𝑖
𝑚𝑖
) , 𝑟𝑖 ≥ 0, 𝑖 = 1, . . . ,6, 
′  are  the  reduced  elastic  moduli,  𝑟𝑖  are  the 
where  𝐸𝑖  are  the  initial  elastic  moduli,  𝐸𝑖
damage  thresholds  computed  from  the  associated  damage  functions  for  fiber  damage, 
matrix  damage  and  delamination,  and  mi  are  material  damage  parameters,  which  are 
currently assumed to be independent of strain-rate.  The damage function is formulated 
to  account  for  the  overall  nonlinear  elastic  response  of  a  lamina  including  the  initial 
‘hardening’ and the subsequent softening beyond the ultimate strengths. 
In  the  damage  model  (material  162),  the  effect  of  strain-rate  on  the  nonlinear  stress-
strain response of a composite layer is modeled by the strain-rate dependent functions 
for the elastic moduli {𝐸𝑅𝑇 } as 
{𝐸𝑅𝑇 } = {𝐸0 } (1 + {𝐶rate} ln 
̇}
{𝜀̅
) 
𝜀̇0
{𝐸𝑅𝑇 } =
⎧ 𝐸𝑎
⎫
}}
{{
𝐸𝑏
}}
{{
𝐸𝑐
⎬
⎨
𝐺𝑎𝑏
}}
{{
𝐺𝑏𝑐
}}
{{
𝐺𝑐𝑎⎭
⎩
{𝜀̅
̇} =
⎧ ∣𝜀̇𝑎∣
⎫
}
{
}
{
∣𝜀̇𝑏∣
}
{
}
{
∣𝜀̇𝑐∣
⎬
⎨
∣𝜀̇𝑎𝑏∣
}
{
}
{
∣𝜀̇𝑏𝑐∣
}
{
}
{
∣𝜀̇𝑐𝑎∣⎭
⎩
{𝐶rate} =
⎧𝐶rate2
⎫
}
{
}
{
𝐶rate2
}
{
}
{
𝐶rate4
⎬
⎨
𝐶rate3
}
{
}
{
𝐶rate3
}
{
}
{
𝐶rate3⎭
⎩
where {𝐶rate} are the strain-rate constants.  {𝐸0 } are the modulus values of {𝐸𝑅𝑇 } at the 
reference strain-rate 𝜀̇0. 
Element Erosion: 
A failed element is eroded in any of three different ways: 
1. 
2. 
3. 
If  fiber  tensile  failure  in  a  unidirectional  layer  is  predicted  in  the  element  and 
the axial tensile strain is greater than E_LIMT.  For a fabric layer, both in-plane 
directions are failed and exceed E_LIMT. 
If compressive relative volume in a failed element is smaller than ECRSH. 
If tensile relative volume in a failed element is greater than EEXPN. 
Damage History Parameters: 
Information about the damage history variables for the associated failure modes can be 
plotted in LS-PrePost.   These additional history variables are tabulated below: 
History 
Variable 
Description 
Value 
LS-PrePost 
History Variable 
1.  efa(I) 
Fiber mode in a 
2.  efb(I) 
Fiber mode in b 
0-elastic 
3.  efp(I) 
Fiber crush mode 
4.  em(I) 
5.  ed(I) 
Perpendicular matrix 
mode 
Parallel matrix/ 
delamination mode 
6.  delm(I) 
delamination mode 
≥1-failed 
7 
8 
9 
10 
11 
12
*MAT_MODIFIED_CRUSHABLE_FOAM 
This is Material Type 163 which is dedicated to modeling crushable foam with optional 
damping,  tension  cutoff,  and  strain  rate  effects.    Unloading  is  fully  elastic.    Tension  is 
treated as elastic-perfectly-plastic at the tension cut-off value. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
TID 
6 
7 
8 
TSC 
DAMP 
NCYCLE 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
0.0 
0.10 
12. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SRCLMT 
SFLAG 
Type 
F 
Default 
1.E+20 
I 
0 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
TID 
TSC 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s modulus 
Poisson’s ratio 
Table  ID  defining  yield  stress  versus  volumetric  strain,  γ,  at 
different strain rates. 
Tensile  stress  cutoff.    A  nonzero,  positive  value  is  strongly
recommended for realistic behavior. 
DAMP 
Rate  sensitivity  via  damping  coefficient  (.05 < recommended 
value<.50).
> >
1-V
Figure  M163-1.    Rate  effects  are  defined  by  a  family  of  curves  giving  yield
stress versus volumetric strain where V is the relative volume. 
  VARIABLE   
DESCRIPTION
NCYCLE 
Number of cycles to determine the average volumetric strain rate.
SRCLMT 
Strain rate change limit. 
SFLAG 
The strain rate in the table may be the true strain rate (SFLAG = 0) 
or the engineering strain rate (SFLAG = 1). 
Remarks: 
The volumetric strain is defined in terms of the relative volume, V, as: 
𝛾 = 1 − V 
The relative volume is defined as the ratio of the current to the initial volume.  In place 
of the effective plastic strain in the D3PLOT database, the integrated volumetric strain is 
output.
This material is an extension of material 63, *MAT_CRUSHABLE_FOAM.  It allows the 
yield stress to be a function of both volumetric strain rate and volumetric strain.  Rate 
effects  are  accounted  for  by  defining  a  table  of  curves  using  *DEFINE_TABLE.    Each 
curve  defines  the  yield  stress  versus  volumetric  strain  for  a  different  strain  rate.    The 
yield  stress  is  obtained  by  interpolating  between  the  two  curves  that  bound  the  strain 
rate. 
To  prevent  high  frequency  oscillations  in  the  strain  rate  from  causing  similar  high 
frequency oscillations in the yield stress, a modified volumetric strain rate is used when 
interpolating to obtain the yield stress.  The modified strain rate is obtained as follows.  
If NYCLE is > 1, then the modified strain rate is obtained by a time average of the actual 
strain rate over NCYCLE solution cycles.  For SRCLMT > 0, the modified strain rate is 
capped  so  that  during  each  cycle,  the  modified  strain  rate  is  not  permitted  to  change 
more than SRCLMT multiplied by the solution time step.
*MAT_BRAIN_LINEAR_VISCOELASTIC 
This is Material Type 164.  This material is a Kelvin-Maxwell model for modeling brain 
tissue, which is valid for solid elements only.  See Remarks below. 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
BULK 
Type 
A8 
F 
F 
4 
G0 
F 
5 
GI 
F 
6 
DC 
F 
7 
FO 
F 
8 
SO 
F 
Default 
none 
none 
none 
none 
none 
0.0 
0.0 
0.0 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density 
BULK 
Bulk modulus (elastic) 
G0 
GI 
DC 
FO 
Short-time shear modulus, G0 
Long-time (infinite) shear modulus, G∞ 
Maxwell decay constant, β[FO = 0.0] or 
Kelvin relaxation constant, τ [FO = 1.0] 
Formulation option: 
EQ.0.0: Maxwell, 
EQ.1.0: Kelvin.
VARIABLE   
SO 
DESCRIPTION
Strain  (logarithmic)  output  option  to  control  what  is  written  as
component 7 to the d3plot database.  (LS-PrePost always blindly 
labels  this  component  as  effective  plastic  strain.)  The  maximum
values are updated for each element each time step: 
EQ.0.0: maximum  principal  strain  that  occurs  during  the
calculation, 
EQ.1.0: maximum magnitude of the principal strain values that
occurs during the calculation, 
EQ.2.0: maximum  effective  strain  that  occurs  during  the
calculation. 
Remarks: 
The shear relaxation behavior is described for the Maxwell model by: 
A Jaumann rate formulation is used 
𝐺(𝑡) = 𝐺 + (𝐺0 − 𝐺∞)𝑒−𝛽𝑡 
𝛻
𝑖𝑗 = 2 ∫ 𝐺(𝑡 − 𝜏)𝐷𝑖𝑗
′ (𝜏)𝑑𝑡 
∇
𝑖𝑗, and the strain rate Dij .  
where the prime denotes the deviatoric part of the stress rate, 𝜎
For the Kelvin model the stress evolution equation is defined as: 
𝑠 ̇𝑖𝑗 +
𝑠𝑖𝑗 = (1 + 𝛿𝑖𝑗)𝐺0𝑒 ̇𝑖𝑗 + (1 + 𝛿𝑖𝑗)
𝐺∞
𝑒 ̇𝑖𝑗 
The  strain  data  as  written  to  the  d3plot  database  may  be  used  to  predict  damage,  see 
[Bandak 1991].
*MAT_PLASTIC_NONLINEAR_KINEMATIC 
This is Material Type 165.  This relatively simple model, based on a material model by 
Lemaitre  and  Chaboche  [1990],  is  suited  to  model  nonlinear  kinematic  hardening 
plasticity.    The  model  accounts  for  the  nonlinear  Bauschinger  effect,  cyclic  hardening, 
and  ratcheting.    Huang  [2006]  programmed  this  model  and  provided  it  as  a  user 
subroutine.  It is a very cost effective model and is available shell and solid elements. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
SIGY 
F 
6 
H 
F 
7 
C 
F 
8 
GAMMA 
F 
Default 
none 
none 
none 
none 
none 
0.0 
0.0 
0.0 
2 
3 
4 
5 
6 
7 
8 
  Card 2 
Variable 
1 
FS 
Type 
F 
Default 
1.E+16 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
SIGY 
Initial yield stress, 𝜎𝑦0. 
H 
C 
Isotropic plastic hardening modulus 
Kinematic hardening modulus
VARIABLE   
DESCRIPTION
GAMMA 
Kinematic hardening parameter, 𝛾. 
FS 
Failure strain for eroding elements. 
Remarks: 
If  the  isotropic  hardening  modulus,  H,  is  nonzero,  the  size  of  the  surface  increases  as 
function of the equivalent plastic strain,𝜀𝑝: 
𝜎𝑦 = 𝜎𝑦0 + 𝐻𝜀𝑝 
The rate of evolution of the kinematic component is a function of the plastic strain rate: 
𝛼̇ = [𝐶𝑛 − 𝛾𝛼]𝜀̇𝑝 
where,  n,  is  the  flow  direction.    The  term,  𝛾𝛼𝜀̇𝑝,  introduces  the  nonlinearity  into  the 
evolution law, which becomes linear if the parameter, 𝛾, is set to zero.
*MAT_PLASTIC_NONLINEAR_KINEMATIC_B 
This  is  Material  Type  165B.    This  material  model  is  implemented  to  model  the  cyclic 
fatigue behavior.  This model applies to both shell and solid elements. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
RE 
F 
6 
B 
F 
7 
Q 
F 
8 
C1 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  GAMMA1 
C2 
GAMMA2
C3 
GAMMA3
Type 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
E 
PR 
RE 
B 
Q 
Mass density. 
Young’s Modulus 
Poisson’s ratio 
Yield stress, see Remarks. 
Material parameter, see Remarks. 
Material parameter, see Remarks.
VARIABLE   
DESCRIPTION
Material parameters, see Remarks.  
C1, 
GAMMA1, 
C2, 
GAMMA2, 
C3, 
GAMMA3 
A model of elastoplatic cyclic hardening: 
This  material  model  is  based  on  a  2013  paper  by  S.    Plessis  which  modeled  a  double-
notched specimen with Herbland (2009) material model.  The elstoplastic stress tensor is 
given by: 
𝜎 = 𝜎𝑀 − 𝐿: ε𝑝 
where, 𝜎𝑀 is elastic stress, ε𝑝 is the plastic strain tensor.  In a one-dimensional problem, 
the above equation becomes: 
where, 𝐿′ is a parameter identified with FEM on a monotonic loading. 
𝜎 = 𝜎𝑀 − 𝐿′ε𝑝 
In the elasticity domain: 
𝑓   = 𝐽2(𝜎 − 𝑋𝑇) − 𝑅𝑒 − 𝑅 ≤ 0 
where  𝐽2  is  the  second  stress  invariant,  𝜎  is  the  stress  tension,  𝑅  is  the  isotropic 
hardening variable, 𝑅𝑒 (variable RE) is the yield stress. 
Evolution law of the isotropic hardening variable R: 
𝑅̇   = 𝑏 𝑋(𝑄 − 𝑅)𝑝̇ 
where  𝑏  (variable  B)  and  𝑄  (variable  Q)  are  two  material  parameters,  𝑝̇  is  the  plastic 
strain rate defined by: 
𝑝̇   = √
𝜖 ̇𝑝: 𝜖 ̇𝑝 
with 𝜖 ̇𝑝 the plastic strain tensor. 
Evolution law of the variable of kinematic hardening: 
with, 
𝑋𝑇̇
  = ∑ 𝑋𝚤̇
𝑋𝚤̇   =
𝐶𝑖𝜖 ̇𝑝 − 𝛾𝑖𝑋𝑖𝑝̇
where 𝑋𝑇̇   is the kinematic hardening tensor, and is the sum of three tensors 𝑋𝚤̇  (𝑖 = 1~3), 
each  dependent  on  the  one  set  of  material  coefficients  𝐶𝑖  (variables  C1,  C2,  C3)  and 
𝛾𝑖(variables GAMMA1, GAMMA2, GAMMA3). 
Revision information: 
This material model is available starting in Revision 102594.
*MAT_MOMENT_CURVATURE_BEAM 
This  is  Material  Type  166.    This  material  is  for  performing  nonlinear  elastic  or  multi-
linear plastic analysis of Belytschko-Schwer beams with user-defined axial force-strain, 
moment  curvature  and  torque-twist  rate  curves.    If  strain,  curvature  or  twist  rate  is 
located  outside  the  curves,  use  extrapolation  to  determine  the  corresponding  rigidity.  
For multi-linear plastic analysis, the user-defined curves are used as yield surfaces. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
5 
6 
7 
8 
ELAF 
EPFLG 
CTA 
CTB 
CTT 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
0.0 
0.0 
0.0 
0.0 
  Card 2 
Variable 
1 
N1 
Type 
F 
2 
N2 
F 
Default 
none 
none 
3 
N3 
F 
0.0 / 
none 
4 
N4 
F 
5 
N5 
F 
6 
N6 
F 
7 
N7 
F 
8 
N8 
F 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCMS1 
LCMS2 
LCMS3 
LCMS4 
LCMS5 
LCMS6 
LCMS7 
LCMS8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
0.0 / 
none 
0.0 
0.0 
0.0 
0.0 
0.0
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCMT1 
LCMT2 
LCMT3 
LCMT4 
LCMT5 
LCMT6 
LCMT7 
LCMT8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
0.0 / 
none 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCT1 
LCT2 
LCT3 
LCT4 
LCT5 
LCT6 
LCT7 
LCT8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
0.0 / 
none 
0.0 
0.0 
0.0 
0.0 
0.0 
Multilinear Plastic Analysis Card.  Additional card for EPFLG = 1. 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CFA 
CFB 
CFT 
HRULE 
REPS 
RBETA 
RCAPAY 
RCAPAZ 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
1.0 
1.0 
1.0 
0.0 
1.0E+20 1.0E+20  1.0E+20  1.0E+20
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s  modulus.    This  variable  controls  the  time  step  size  and
must be chosen carefully.  Increasing the value of E will decrease
the time step size.
VARIABLE   
DESCRIPTION
ELAF 
Load curve ID for the axial force-strain curve 
EPFLG 
Function flag 
EQ.0.0: nonlinear elastic analysis 
EQ.1.0: multi-linear plastic analysis 
CTA, CTB, 
CTT 
Type  of  axial  force-strain,  moment-curvature,  and  torque-twist 
rate curves 
EQ.0.0: curve is symmetric 
EQ.1.0: curve is asymmetric 
For symmetric curves, all data point must be in the first quadrant 
and at least three data points need to be given, starting from the
origin, ensued by the yield point.   
For  asymmetric  curves,  at  least  five  data  points  are  needed  and
exactly  one  point  must  be  at  the origin.   The  two  points  on  both
sides of the origin record the positive and negative yield points. 
The last data point(s) has no physical meaning: it serves only as a
control point for inter or extrapolation. 
The  curves  are  input  by  the  user  and  treated  in  LS-DYNA  as  a 
linearly  piecewise  function.    The  curves  must  be  monotonically 
increasing, while the slopes must be monotonically decreasing 
Axial  forces  at  which  moment-curvature  curves  are  given.    The 
axial  forces  must  be  ordered  monotonically  increasing.    At  least
two axial forces must be defined if the curves are symmetric.  At 
least  three  axial  forces  must  be  defined  if  the  curves  are
asymmetric. 
Load  curve  IDs  for  the  moment-curvature  curves  about  axis  S 
under corresponding axial forces. 
Load  curve  IDs  for  the  moment-curvature  curves  about  axis  T 
under corresponding axial forces. 
Load  curve 
corresponding axial forces. 
IDs 
for 
the 
torque-twist  rate  curves  under 
For multi-linear plastic analysis only.  Ratio of axial, bending and
torsional elastic rigidities to their initial values, no less than 1.0 in
value. 
N1 - N8 
LCMS1 - 
LCMS8 
LCMT1 - 
LCMT8 
LCT1 - LCT8 
CFA, CFB, 
CFT
*MAT_MOMENT_CURVATURE_BEAM 
DESCRIPTION
HRULE 
Hardening rule, for multi-linear plastic analysis only. 
EQ.0.0: 
isotropic hardening 
GT.0.0.AND.LT.1.0: mixed hardening 
EQ.1.0: 
kinematic hardening 
REPS 
Rupture effective plastic axial strain 
RBETA 
Rupture effective plastic twist rate 
RCAPAY 
Rupture effective plastic curvature about axis S 
RCAPAZ 
Rupture effective plastic curvature about axis T
*MAT_167 
This  is  Material  Type  167.    This  is  a  constitute  model  for  finite  plastic  deformities  in 
which  the  material’s  strength  is  defined  by  McCormick’s  constitutive  relation  for 
materials  exhibiting  negative  steady-state  Strain  Rate  Sensitivity  (SRS).    McCormick 
[1988] and Zhang, McCormick and Estrin [2001]. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
  Card 2 
Variable 
1 
Q1 
Type 
F 
  Card 3 
Variable 
Type 
1 
S 
F 
2 
C1 
F 
2 
H 
F 
3 
E 
F 
3 
Q2 
F 
3 
4 
PR 
F 
4 
C2 
F 
4 
5 
6 
7 
8 
SIGY 
F 
5 
6 
7 
8 
5 
6 
7 
8 
OMEGA 
TD 
ALPHA 
EPS0 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
Material identification. A unique number or label not exceeding 8 
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
SIGY 
Initial yield stress 
Q1 
C1 
Isotropic hardening parameter, 𝑄1 
Isotropic hardening parameter, 𝐶1
VARIABLE   
Q2 
C2 
S 
H 
DESCRIPTION
Isotropic hardening parameter, 𝑄2 
Isotropic hardening parameter, 𝐶2 
Dynamic strain aging parameter, 𝑆 
Dynamic strain aging parameter, 𝐻 
OMEGA 
Dynamic strain aging parameter, Ω 
TD 
Dynamic strain aging parameter, 𝑡𝑑 
ALPHA 
Dynamic strain aging parameter, 𝛼 
EPS0 
Reference strain rate, 𝜀̇0 
Remarks: 
The uniaxial stress-strain curve is given in the following form: 
𝜎(𝜀𝑝, 𝜀̇𝑝) = 𝜎𝑌(𝑡𝑎) + 𝑅(𝜀𝑝) + 𝜎𝑣(𝜀̇𝑝) 
Viscous stress 𝜎𝑣 is given by  
𝜎𝑣(𝜀̇𝑝) = S × ln (1 +
𝜀̇𝑝
𝜀̇𝑜
) 
where 𝑆 represents the instantaneous strain rate sensitivity and 𝜀̇𝑜 is a reference strain 
rate. 
In  the  McCormick  model  the  yield  strength  including  the  contribution  from  dynamic 
strain again (DSA) is defined as 
𝜎𝑌(𝑡𝑎) = 𝜎𝑜 + S × H × [1 − exp {− (
)
𝑡𝑎
𝑡𝑑
}] 
where 𝜎𝑜 is the yield strength for vanishing average waiting time 𝑡𝑎, and 𝐻, 𝛼, and 𝑡𝑑 are 
material constants linked to dynamic strain aging. 
The average waiting time is defined by the evolution equation 
𝑡 ̇𝑎 = 1 −
𝑡𝑎
𝑡𝑎,𝑠𝑠
where the quasi-steady state waiting time 𝑡𝑎,𝑠𝑠 is given as 
𝑡𝑎,𝑠𝑠 =
𝜀̇𝑝.
The strain hardening function 𝑅 is defined by the extended Voce Law 
𝑅(𝜀𝑝) = 𝑄1[1 − exp(−𝐶1𝜀𝑝)] + 𝑄2[1 − exp(−𝐶2𝜀𝑝)].
*MAT_POLYMER 
This is material type 168.  This model is implemented for brick elements. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
Variable 
TEMP 
Type 
F 
2 
RO 
F 
2 
K 
F 
3 
E 
F 
3 
CR 
F 
4 
5 
6 
PR 
GAMMA0
DG 
F 
6 
F 
4 
N 
F 
F 
5 
C 
F 
  VARIABLE   
DESCRIPTION
7 
SC 
F 
7 
8 
ST 
F 
8 
MID 
RO 
E 
PR 
Material identification. A unique number or label not exceeding 8 
characters must be specified. 
Mass Density. 
Young’s modulus, 𝐸. 
Poisson’s ratio, 𝜈. 
GAMMA0 
Pre-exponential factor, 𝛾̇0𝐴. 
DG 
SC 
ST 
Energy barrier to flow, Δ𝐺. 
Shear resistance in compression, 𝑆𝑐. 
Shear resistance in tension, 𝑆𝑡. 
TEMP 
Absolute temperature, 𝜃. 
K 
CR 
N 
C 
Boltzmann constant, 𝑘. 
Product, 𝐶𝑟 = 𝑛𝑘𝜃. 
Number of ‘rigid links’ between entanglements, 𝑁. 
Relaxation factor, 𝐶.
*MAT_168 
The polymer is assumed to have two basic resistances to deformation: 
Elastic stiffness
(Hooke's law)
Plastic flow
(Argon's model)
A B
Network
stiffness
(Arruda-
Boyce model)
Total
A  (Inter-molecular)
B  (Network)
True strain
Figure  M168-1.    Stress  decomposition  in  inter-molecular  and  network
contributions. 
1.  An  inter-molecular  barrier  to  deformation  related  to  relative  movement 
between molecules. 
2.  An  evolving  anisotropic  resistance  related  to  straightening  of  the  molecule 
chains. 
The  model  which  is  implemented  and  presented  in  this  paper  is  mainly  based  on  the 
framework  suggested  by  Boyce  et  al.    [2000].    Going  back  to  the  original  work  by 
Haward and Thackray [1968], they considered the uniaxial case only.  The extension to 
a  full  3D  formulation  was  proposed  by  Boyce  et  al.    [1988].    Moreover,  Boyce  and  co-
workers have during a period of 20 years changed or further developed the parts of the 
original  model.    Haward  and  Thackray  [1968]  used  an  Eyring  model  to  represent  the 
dashpot in Fig. M168-1, while  Boyce et al.  [2000] employed the double-kink model of 
Argon  [1973]  instead.    Part  B  of  the  model,  describing  the  resistance  associated  with 
straightening of the molecules, contained originally a one-dimensional Langevin spring 
[Haward and Thackray, 1968], which was generalized to 3D with the eight-chain model 
by Arruda and Boyce [1993]. 
The main structure of the model presented by Boyce et al.  [2000] is kept for this model.  
Recognizing the large elastic deformations occurring for polymers, a formulation based
on a Neo-Hookean material is here selected for describing the spring in resistance A in 
Figure M168-1. 
Referring  to  Figure  M168-1,  it  is  assumed  that  the  deformation  gradient  tensor  is  the 
same for the two resistances (Part A and B) 
while the Cauchy stress tensor for the system is assumed to be the sum of the Cauchy 
stress tensors for the two parts 
𝐅 = 𝐅𝐴 = 𝐅𝐵 
σ = σ𝐴 + σ𝐵. 
Part A: Inter-molecular resistance: 
𝑝 , where it is 
The deformation is decomposed into elastic and plastic parts, 𝐅𝐴 = 𝐅𝐴
𝑝   is  invariant  to  rigid 
assumed  that  the  intermediate  configuration  Ω̅̅̅̅̅̅𝐴  defined  by  𝐅𝐴
body  rotations  of  the  current  configuration.    The  velocity  gradient  in  the  current 
configuration Ω is defined by 
𝑒 ⋅ 𝐅𝐴
Owing  to  the  decomposition,  𝐅𝐴 = 𝐅𝐴
and spin tensors are defined by 
𝐋𝐴 = 𝐅̇𝐴 ⋅ 𝐅𝐴
𝑒 ⋅ 𝐅𝐴
𝑝  
𝑒 + 𝐋𝐴
−1 = 𝐋𝐴
𝑝 ,  the  elastic  and  plastic  rate-of-deformation 
𝑒 + 𝐖𝐴
𝑝 + 𝐖𝐴
𝑒 = 𝐅̇
𝑝 = 𝐅𝐴
𝑒 ⋅ (𝐅𝐴
𝑒 ⋅ 𝐅̇
𝑒 )−1
𝑝 ⋅ (𝐅𝐴
𝑝 )−1 ⋅ (𝐅𝐴
𝑒 )−1 = 𝐅𝐴
𝑒 ⋅ 𝐋̅
𝑝 ⋅ (𝐅𝐴
𝑒 )−1 
𝑒 = 𝐃𝐴
𝐋𝐴
𝑝 = 𝐃𝐴
𝐋𝐴
𝑝 ⋅ (𝐅𝐴
𝑝 = 𝐅̇
𝑝 )−1. The Neo-Hookean material represents an extension of Hooke's 
where 𝐋̅
law  to  large  elastic  deformations  and  may  be  chosen  for  the  elastic  part  of  the 
deformation when the elastic behavior is assumed to be isotropic. 
τ𝐴 = 𝜆0ln𝐽𝐴
𝑒   𝐈 + 𝜇0(𝐁𝐴
𝑒 − 𝐈) 
𝑒 = 𝐽𝐴   is  the 
where τ𝐴 = 𝐽𝐴σ𝐴  is  the  Kirchhoff  stress  tensor  of  Part  A  and  𝐽𝐴
Jacobian  determinant.    The  elastic  left  Cauchy-Green  deformation  tensor  is  given  by 
𝑒 = 𝐅𝐴
𝐁𝐴
𝑒 = √det𝐁𝐴
𝑒 ⋅ 𝐅𝐴
𝑒 𝑇. 
The flow rule is defined by 
where 
𝑝 = 𝛾̇𝐴
𝐋𝐴
𝑝 𝐍𝐴 
𝐍𝐴 =
√2 𝜏𝐴
dev,
τ𝐴
𝜏𝐴 = √
dev)
tr(τ𝐴
𝑑𝑒𝑣  is  the  stress  deviator.    The  rate  of  flow  is  taken  to  be  a  thermally  activated 
and  τ𝐴
process
𝑝 = 𝛾̇0𝐴exp [−
𝛾̇𝐴
Δ𝐺(1 − 𝜏𝐴/𝑠)
𝑘𝜃
] 
where  𝛾̇0𝐴  is  a  pre-exponential  factor,  Δ𝐺  is  the  energy  barrier  to  flow,  𝑠  is  the  shear 
resistance,  𝑘  is  the  Boltzmann  constant  and  𝜃  is  the  absolute  temperature.    The  shear 
resistance 𝑠 is assumed to depend on the stress triaxiality 𝜎 ∗, 
𝑠 = 𝑠(𝜎 ∗),    𝜎 ∗ =
tr σ𝐴
3√3𝜏𝐴
The exact dependence is given by a user-defined load curve, which is linear between the 
shear  resistances  in  compression  and  tension.    These  resistances  are  denoted  sc  and  st, 
respectively. 
Part B: Network resistance: 
The  network  resistance  is  assumed  to  be  nonlinear  elastic  with  deformation  gradient 
𝑁,  i.e.    any  viscoplastic  deformation  of  the  network  is  neglected.    The  stress-
𝐅𝐵 = 𝐅𝐵
stretch relation is defined by 
τ𝐵 =
𝑛𝑘𝜃
√𝑁
𝜆̅̅̅̅𝑁
ℒ −1
⎜⎛ 𝜆̅̅̅̅𝑁
√𝑁⎠
⎝
⎟⎞ (𝐁̅̅̅̅
𝑁 − 𝜆̅̅̅̅
2 𝐈) 
where  τ𝐵 = 𝐽𝐵σ𝐵  is  the  Kirchhoff  stress  for  Part  B,  𝑛  is  the  chain  density  and  𝑁  the 
number of ‘rigid links’ between entanglements.  In accordance with Boyce et.  al [2000], 
the product, 𝑛𝑘𝜃 is denoted  𝐶𝑅 herein.  Moreover, ℒ −1 is the inverse Langevin function, 
ℒ(𝛽) = coth𝛽 − 1 𝛽⁄ , and further 
𝐁̅̅̅̅
𝑁 = 𝐅̅̅̅̅
𝑁 ⋅ 𝐅̅̅̅̅
𝑁 𝑇
,    𝐅̅̅̅̅
𝑁 = 𝐽𝐵
−1/3 𝐅𝐵
𝑁,    𝐽𝐵 = det𝐅𝐵
𝑁,    𝜆̅̅̅̅𝑁 = [
tr 𝐁̅̅̅̅
𝑁]
The flow rule defining the rate of molecular relaxation reads 
𝐹 = 𝛾̇𝐵
𝐋𝐵
𝐹𝐍𝐵 
where 
𝐍𝐵 =
√2 𝜏𝐵
dev,
τ𝐵
𝜏𝐵 = √
dev: τ𝐵
τ𝐵
dev 
The rate of relaxation is taken equal to 
where 
𝐹 = 𝐶 (
𝛾̇𝐵
𝜆̅̅̅̅𝐹 − 1
) 𝜏𝐵 
𝜆̅̅̅̅𝐹 = [
tr(𝐅𝐵
𝐹}
𝐹{𝐅𝐵
)]
The  model  has  been  implemented  into  LS-DYNA  using  a  semi-implicit  stress-update 
scheme [Moran et.  al 1990], and is available for the explicit solver only.
*MAT_169 
This  is  Material  Type  169.    This  material  model  was  written  for  adhesive  bonding  in 
aluminum structures.  The plasticity model is not volume-conserving, and hence avoids 
the  spuriously  high  tensile  stresses  that  can  develop  if  adhesive  is  modeled  using 
traditional  elasto-plastic  material  models.    It  is  available  only  for  solid  elements  of 
formulations 1, 2 and 15.   The smallest dimension of the element is assumed to be the 
through-thickness dimension of the bond, unless THKDIR = 1. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
5 
6 
7 
8 
PR 
TENMAX 
GCTEN 
SHRMAX 
GCSHR 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
1020 
1020 
1020 
1020 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PWRT 
PWRS 
SHRP 
SHT_SL 
EDOT0 
EDOT2 
THKDIR 
EXTRA 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
2.0 
2.0 
0.0 
0.0 
1.0 
0.0 
0.0 
0.0 
Additional card for Extra = 1 or 3.  
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TMAXE 
GCTE 
SMAXE 
GCSE 
PWRTE 
PWRSE 
Type 
F 
F 
F 
F 
F 
F 
Default 
1020 
1020 
1020 
1020 
2.0 
2.0
*MAT_ARUP_ADHESIVE 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FACET 
FACCT 
FACES 
FACCS 
SOFTT 
SOFTS 
Type 
F 
F 
F 
F 
F 
F 
Default 
1.0 
1.0 
1.0 
1.0 
1.0 
1.0 
Dynamic Strain Rate Card.  Additional card for EDOT2 ≠ 0. 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SDFAC 
SGFAC 
SDEFAC 
SGEFAC 
Type 
F 
F 
F 
F 
Default 
1.0 
1.0 
1.0 
1.0 
Bond Thickness Card.  Additional card for Extra = 2 or 3. 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BTHK 
OUTFAIL 
FSIP 
Type 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
Material identification. A unique number or label not exceeding 8 
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio.
VARIABLE   
DESCRIPTION
TENMAX 
Maximum through-thickness tensile stress  
GT.0.0:  constant value 
LT.0.0:  |TENMAX|  is  ID  of  a  *DEFINE_FUNCTION   
GCTEN 
Energy per unit area to fail the bond in tension  
GT.0.0:  constant value 
LT.0.0:  |GCTEN|  is  ID  of  a  *DEFINE_FUNCTION   
SHRMAX 
Maximum through-thickness shear stress  
GT.0.0:  constant value 
LT.0.0:  |SHRMAX|  is  ID  of  a  *DEFINE_FUNCTION   
GCSHR 
Energy per unit area to fail the bond in shear  
GT.0.0:  constant value 
LT.0.0:  |GCSHR|  is  ID  of  a  *DEFINE_FUNCTION   
Power law term for tension 
Power law term for shear 
Shear plateau ratio (Optional)  
GT.0.0:  constant value 
LT.0.0:  |SHRP| 
Remarks) 
is 
ID  of  a  *DEFINE_FUNCTION 
  of  yield  surface  at  zero  tension   
EDOT0 
Strain rate at which the “static” properties apply 
EDOT2 
Strain rate at which the “dynamic” properties apply (Card 5) 
THKDIR 
Through-thickness direction flag  
EQ.0.0: smallest element dimension (default) 
EQ.1.0: direction from nodes 1-2-3-4 to nodes 5-6-7-8
*MAT_ARUP_ADHESIVE 
DESCRIPTION
EXTRA 
Flag to input further data: 
EQ.1.0: interfacial failure properties (cards 3 and 4) 
EQ.2.0: bond thickness and more (card 6) 
EQ.3.0: both of the above 
TMAXE 
Maximum tensile force per unit length on edges of joint 
GCTE 
Energy per unit length to fail the edge of the bond in tension 
SMAXE 
Maximum shear force per unit length on edges of joint 
GCSE 
Energy per unit length to fail the edge of the bond in shear 
PWRTE 
Power law term for tension 
PWRSE 
Power law term for shear 
FACET 
Stiffness scaling factor for edge elements – tension 
FACCT 
Stiffness scaling factor for interior elements – tension 
FACES 
Stiffness scaling factor for edge elements – shear 
FACCS 
Stiffness scaling factor for interior elements – shear 
SOFTT 
SOFTS 
Factor by which the tensile strength is reduced when a neighbor
fails 
Factor  by  which  the  shear  strength  is  reduced  when  a  neighbor 
fails 
SDFAC 
Factor on TENMAX and SHRMAX at strain rate EDOT2  
GT.0.0:  constant value 
LT.0.0:  |SDFAC| 
Remarks) 
is  ID  of  a  *DEFINE_FUNCTION   
is  ID  of  a  *DEFINE_FUNCTION  (see
SDEFAC 
Factor on TMAXE and SMAXE at strain rate EDOT2
VARIABLE   
DESCRIPTION
SGEFAC 
Factor on GCTE and GCSE at strain rate EDOT2 
BTHK 
Bond thickness (overrides thickness from element dimensions)  
LT.0.0: |BTHK|  is  bond  thickness,  but  critical  time  step
remains  unaffected.    Helps  to  avoid  very  small  time
steps, but it can affect stability. 
OUTFAIL 
Flag  for  additional  output  to  messag  file:  Information  about
damage 
initiation time, failure function terms and forces. 
EQ.0.0: off 
EQ.1.0: on 
FSIP 
Effective in-plane strain at failure. 
Remarks: 
The  through-thickness  direction  is  identified  from  the  smallest  dimension  of  each 
element  by  default  (THKDIR = 0.0).    It  is  expected  that  this  dimension  will  be  smaller 
than  in-plane  dimensions  (typically  1-2mm  compared  with  5-10mm).  If  this  is  not  the 
through-thickness  direction  via  element  numbering 
case,  one  can  set 
(THKDIR = 1.0).    Then  the  thickness  direction  is  expected  to  point  from  lower  face 
(nodes  1-2-3-4)  to  upper  face  (nodes  5-6-7-8).    For  wedge  elements  these  faces  are  the 
two triangular faces (nodes 1-2-5) and (nodes 3-4-6). 
the 
The  bond  thickness  is  assumed  to  be  the  element  size  in  the  thickness  direction.    This 
may be overridden using BTHK.  In this case the behavior becomes independent of the 
element thickness.  The elastic stiffness is affected by BTHK, so it is necessary to set the 
characteristic element length to a smaller value 
new = √BTHK × 𝑙𝑒
𝑙𝑒
old. 
This again affects the critical time step of the element, i.e.  a small BTHK can decrease 
the element time step significantly. 
In-plane  stresses  are  set  to  zero:  it  is  assumed  that  the  stiffness  and  strength  of  the 
substrate is large compared with that of the adhesive, given the relative thicknesses. 
If  the  substrate  is  modeled  with  shell  elements,  it  is  expected  that  these  will  lie  at  the 
mid-surface  of  the  substrate  geometry.    Therefore  the  solid  elements  representing  the 
adhesive  will  be  thicker  than the  actual  bond.    If the  elastic  compliance  of  the  bond  is 
significant, this can be corrected by increasing the elastic stiffness property E.
SHT_SL > 0
SHT_SL = 0
shear
stress
SHRMAX
direct
stress
TENMAX
Figure M169-1.  Figure illustrating the yield surface. 
The yield and failure surfaces are treated as a power-law combination of direct tension 
and shear across the bond: 
(
𝜎max
PWRT
     + (
)
𝜏max − SHT_ SL × 𝜎
PWRS
     = 1.0 
)
At yield SHT_SL is the slope of the yield surface at 𝜎 = 0.  See Figure M169-1 
The  stress-displacement  curves  for  tension  and  shear  are  shown  in Figure  M169-2.    In 
both  cases,  GC  is  the  area  under  the  curve.    The  displacement  to  failure  in  tension  is 
given by 
subject to a lower limit 
𝑑ft = 2 (
GCTEN
TENMAX
) , 
𝑑ft, min = (
2𝐿0
𝐸′ ) TENMAX 
where 𝐿0 is the initial element thickness (or BTHK if used) and 
𝐸′ =
𝐸(1 − 𝜈)
(1 − 2𝜈)(1 + 𝜈)
 . 
If GCTEN is input such that 𝑑ft < 𝑑ft, min, LS-DYNA will automatically increase GCTEN 
to make 𝑑ft = 𝑑ft, min.  Therefore, GCTEN has a minimum value of 
dp = SHRP × dfs
TENAMX
Area = GCten
Failure (dft)
SHRMAX
Area = GCshr
Failure (dfs)
Displacement
(Tension)
Displacement
(Shear)
Figure M169-2.  Stress-Displacement Curves for Tension and Shear.
σMAX/TENMAX 
SDFAC 
1.0 
Log(plastic strain rate) 
Log(EDOT0) 
Log(EDOT2) 
Figure M169-3.  Figure illustrating rate effects. 
Similarly, the minimum value for GCSHR is 
GCTEN ≥
𝐿0
𝐸′ (TENMAX)2 
GCSHR ≥
𝐿0
(SHRMAX)2 
where 𝐺 is the elastic shear modulus. 
Because  of  the  algorithm  used,  yielding  in  tension  across  the  bond  does  not  require 
strains in the plane of the bond – unlike the plasticity models, plastic flow is not treated 
as volume-conserving. 
The Plastic Strain output variable has a special meaning: 
0 < PS < 1:  PS  is  the  maximum  value  of  the  yield  function  experienced 
since time zero 
1 < PS < 2: 
the element has yielded and the strength is reducing towards 
failure – yields at PS = 1, fails at PS = 2. 
The  damage  cause  by  cohesive  deformation  (0  at  first  yield  to  1  at  failure)  and  by 
interfacial deformation are stored in the first two extra history variables.  These can be 
plotted if NEIPH on *DATABASE_EXTENT_BINARY is 2 or more.  By this means, the 
reasons for failure may be assessed. 
When the plastic  strain rate rises above EDOT0, rate effects are assumed to scale with 
the  logarithm  of  the  lastic  strain  rate,  as  in  the  example  shown  in  Figure  M169-3  for 
cohesive tensile strength with dynamic factor SDFAC.  The same form of relationship is 
applied  for  the  other  dynamic  factors.    If  EDOT0  is  zero  or  blank,  no  rate  effects  are 
applied.  Rate effects are applied using the viscoplastic method.
Interfacial failure is assumed to arise from stress concentrations at the edges of the bond 
– typically the strength of the bond becomes almost independent of bond length.  This 
type of failure is usually more brittle than cohesive failure.  To simulate this, LS-DYNA 
identifies the free edges of the bond (made  up of element faces that are not shared by 
other  elements  of  material  type  *MAT_ARUP_ADHESIVE,  excluding  the  faces  that 
bond  to  the  substrate).    Only these  elements  can  fail  initially.    The  neighbors  of  failed 
elements can then develop free edges and fail in turn. 
In  real  adhesive  bonds,  the  stresses  at  the  edges  can  be  concentrated  over  very  small 
areas; in typical finite element models the elements are much too large to capture this.  
Therefore  the  concentration  of  loads  onto  the  edges  of  the  bond  is  accomplished 
artificially,  by  stiffening  elements  containing  free  edges  (e.g.    FACET,  FACES > 1)  and 
reducing the stiffness of interior elements (e.g.  FACCT, FACCS < 1).  Interior elements 
are  allowed  to  yield  at  reduced  loads  (equivalent  to  TMAXE × FACET/FACCT  and 
SMAXE × FACES/FACCS)  to  prevent  excessive  stresses  developing  before  the  edge 
elements have failed - but cannot be damaged until they become edge elements after the 
failure of their neighbors. 
Parameters TENMAX, GCTEN, SHRMAX, GCSHR, SHRP, SDFAC, and SGFAC can be 
defined  as  negative  values. 
to 
*DEFINE_FUNCTION  ID’s.    The  arguments  of  those  functions  include  several 
properties  of  both  connection  partners  if  corresponding  solid  elements  are  in  a  tied 
contact with shell elements. 
the  absolute  values  refer 
that  case, 
In 
These functions depend on: 
(t1, t2) = thicknesses of both bond partners 
(sy1, sy2) = initial yield stresses at plastic strain of 0.002 
(sm1, sm2) = maximum engineering yield stresses (necking points) 
r = strain rate 
a = element area 
For TENMAX  =  -100 such a function could look like: 
*DEFINE_FUNCTION 
        100 
 func(t1,t2,sy1,sy2,sm1,sm2,r,a)=0.5*(sy1+sy2) 
Since  material  parameters  have  to  be  identified  from  both  bond  partners  during 
initialization,  this  feature  is  only  available  for  a  subset  of  material  models  at  the 
moment, namely no.  24, 120, 123, and 124.
*MAT_RESULTANT_ANISOTROPIC 
This  is  Material  Type  170.    This  model  is  available  the  Belytschko-Tsay  and  the  C0 
triangular  shell  elements  and  is  based  on  a  resultant  stress  formulation.    In-plane 
behavior is treated separately from bending in order to model perforated materials such 
as television shadow  masks.   The plastic behavior of each resultant is specified  with a 
load  curve  and  is  completely  uncoupled  from  the  other  resultants.    If  other  shell 
formulations  are  specified,  the  formulation  will  be  automatically  switched  to 
Belytschko-Tsay.    As  implemented,  this  material  model  cannot  be  used  with  user 
defined integration rules. 
NOTE: This material does not support specification of a ma-
terial  angle,  𝛽𝑖,  for  each  through-thickness  integra-
tion point of a shell. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
4 
5 
6 
7 
8 
3 
4 
5 
6 
7 
8 
Variable 
E11P 
E22P 
V12P 
V21P 
G12P 
G23P 
G31P 
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
8 
Variable 
E11B 
E22B 
V12B 
V21B 
G12B 
AOPT 
Type 
F 
F 
F 
F 
F
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LN11 
LN22 
LN12 
LQ1 
LQ2 
LM11 
LM22 
LM12 
Type 
F 
  Card 5 
1 
Variable 
Type 
  Card 6 
Variable 
1 
V1 
Type 
F 
F 
2 
2 
V2 
F 
F 
3 
3 
V3 
F 
F 
F 
F 
4 
A1 
F 
4 
D1 
F 
5 
A2 
F 
5 
D2 
F 
6 
A3 
F 
6 
D3 
F 
F 
7 
F 
8 
7 
8 
BETA 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E11P 
E22P 
V12P 
V11P 
G12P 
G23P 
G31P 
E11B 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
𝐸11𝑝, for in plane behavior. 
𝐸22𝑝, for in plane behavior. 
𝜈12𝑝, for in plane behavior. 
𝜈11𝑝, for in plane behavior. 
𝐺12𝑝, for in plane behavior. 
𝐺23𝑝, for in plane behavior. 
𝐺31𝑝, for in plane behavior. 
𝐸11𝑏, for bending behavior.
VARIABLE   
DESCRIPTION
E22B 
V12B 
V21B 
G12B 
AOPT 
𝐸22𝑏, for bending behavior. 
𝜈12𝑏, for bending behavior. 
𝜈21𝑏, for bending behavior. 
𝐺12𝑏, for bending behavior. 
Material  axes  option  : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by 
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES,  and  then  rotated  about  the  shell  ele-
ment normal by the angle BETA. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  𝐯  with  the
element normal. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
LN11 
LN22 
LN12 
LQ1 
LQ2 
LM11 
LM22 
LM12 
Yield curve ID for 𝑁11, the in-plane force resultant. 
Yield curve ID for 𝑁22, the in-plane force resultant. 
Yield curve ID for 𝑁12, the in-plane force resultant. 
Yield curve ID for 𝑄1, the transverse shear resultant. 
Yield curve ID for 𝑄2, the transverse shear resultant. 
Yield curve ID for 𝑀11, the moment. 
Yield curve ID for 𝑀22, the moment. 
Yield curve ID for 𝑀12, the moment.
*MAT_RESULTANT_ANISOTROPIC 
DESCRIPTION
A1, A2, A3 
(𝑎1, 𝑎2, 𝑎3), define components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
(𝑣1, 𝑣2, 𝑣3), define components of vector 𝐯 for AOPT = 3. 
D1, D2, D3 
(𝑑1, 𝑑2, 𝑑3), define components of vector 𝐝 for AOPT = 2. 
BETA 
Material angle in degrees for AOPT = 0 and 3, may be overridden 
on the element card, see *ELEMENT_SHELL_BETA. 
Remarks: 
The in-plane elastic matrix for in-plane, plane stress behavior is given by: 
𝐂in plane =
𝑄11𝑝        𝑄12𝑝      0        0        0
⎤
𝑄12𝑝        𝑄22𝑝      0        0        0
⎥
⎥
    0          0        𝑄44𝑝      0        0
⎥
⎥
    0          0        0        𝑄55𝑝      0
⎥
    0          0        0        0        𝑄66𝑝⎦
⎡
⎢
⎢
⎢
⎢
⎢
⎣
The terms 𝑄𝑖𝑗𝑝 are defined as: 
𝑄11𝑝 =
𝑄22𝑝 =
𝑄12𝑝 =
𝐸11𝑝
1 − 𝜈12𝑝𝜈21𝑝
𝐸22𝑝
1 − 𝜈12𝑝𝜈21𝑝
𝜈12𝑝𝐸11𝑝
1 − 𝜈12𝑝𝜈21𝑝
𝑄44𝑝 = 𝐺12𝑝 
𝑄55𝑝 = 𝐺23𝑝 
𝑄66𝑝 = 𝐺31𝑝 
The elastic matrix for bending behavior is given by: 
𝐂bending =
𝑄11𝑏        𝑄12𝑏      0
⎤
⎡
𝑄12𝑏        𝑄22𝑏      0
⎥
⎢
    0          0        𝑄44𝑏⎦
⎣
The terms 𝑄𝑖𝑗𝑝 are similarly defined. 
Because this is a resultant formulation, no stresses are output to d3plot, and forces and 
moments are reported to elout in place of stresses.
*MAT_STEEL_CONCENTRIC_BRACE 
This is Material Type 171.  It represents the cyclic buckling and tensile yielding behavior 
of  steel  braces  and  is  intended  primarily  for  seismic  analysis.    Use  only  for  beam 
elements with ELFORM = 2 (Belytschko-Schwer beam). 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
YM 
Type 
A8 
F 
F 
4 
PR 
F 
5 
6 
7 
8 
SIGY 
LAMDA 
FBUCK 
FBUCK2 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
See 
Remarks 
See 
Remarks 
0.0 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CCBRF 
BCUR 
Type 
F 
F 
Default 
See 
Remarks 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TS1 
TS2 
TS3 
TS4 
CS1 
CS2 
CS3 
CS4 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
F 
F 
F 
 = TS1 
 = TS2 
 = TS3 
 = TS4 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density
VARIABLE   
DESCRIPTION
YM 
PR 
Young’s Modulus 
Poisson’s Ratio 
SIGY 
Yield stress 
LAMDA 
Slenderness ratio (optional – see note) 
FBUCK 
Initial  buckling  load  (optional  –  see  note.    If  used,  should  be 
positive) 
FBUCK2 
Optional extra term in initial buckling load – see note 
CCBRF 
Reduction factor on initial buckling load for cyclic behavior 
BCUR 
Optional  load  curve  giving  compressive  buckling  load  (y-axis) 
versus compressive strain (x-axis - both positive) 
TS1 - TS4 
Tensile axial strain thresholds 1 to 4 
CS1 - CS4 
Compressive axial strain thresholds 1 to 4 
Remarks: 
The brace element is intended to represent the buckling, yielding and cyclic behavior of 
steel  elements  such  as  tubes  or  I-sections  that  carry  only  axial  loads.    Empirical 
relationships are used to determine the buckling and cyclic load-deflection behavior.  A 
single beam element should be used to represent each structural element. 
The  cyclic  behavior  is  shown  in  the  graph  (compression  shown  as  negative  force  and 
displacement).
16
17
15
12
19 
14 
11,13
10
18
Figure M171-1.  
The initial buckling load (point 2) is: 
𝐹𝑏  initial = FBUCK +
FBUCK2
𝐿2
where FBUCK, FBUCK2 are input parameters and L is the length of the beam element.  
If neither FBUCK nor FBUCK2 are defined, the default is that the initial buckling load is  
where A is the cross sectional area.  The buckling curve (shown dashed) has the form: 
SIGY × A, 
𝐹(𝑑) =
𝐹b initial
√𝐴𝛿 + 𝐵
where  𝛿  is  abs(strain/yield  strain),  and  A  and  B  are  internally-calculated  functions  of 
slenderness ratio (λ) and loading history. 
The member slenderness ratio λ is defined as 𝑘𝐿
𝑟 , where k depends on end conditions, L 
is  the  element  length,  and  r  is  the  radius  of  gyration  such  that  𝐴𝑟2 = 𝐼  (and  𝐼 =
min(𝐼𝑦𝑦, 𝐼𝑧𝑧)); λ  will  by  default  be  calculated  from  the  section  properties  and  element 
length using k = 1.  Optionally, this may be overridden by input parameter LAMDA to 
allow for different end conditions. 
Optionally, the user may provide a buckling curve BCUR.  The points of the curve give 
compressive displacement (x-axis) versus force (y-axis); the first point should have zero 
displacement  and  the  initial  buckling  force.    Displacement  and  force  should  both  be 
positive.  The initial buckling force must not be greater than the yield force.
The tensile yield force (point 5 and section 16-17) is defined by 
𝐹𝑦 = SIGY × 𝐴, 
where yield stress SIGY is an input parameter and A is the cross-sectional area. 
Following  initial  buckling  and  subsequent  yield  in  tension,  the  member  is  assumed  to 
be  damaged.    The  initial  buckling  curve  is  then  scaled  by  input  parameter  CCBRF, 
leading  to  reduced  strength  curves  such  as  segments  6-7,  10-14  and  18-19.    This 
reduction  factor  is  typically  in  the  range  0.6  to  1.0  (smaller  values  for  more  slender 
members).  By default, CCBRF is calculated using SEAOC 1990: 
CCBRF =
⎜⎜⎜⎛1 + 0.5𝜆
𝜋√
⎟⎟⎟⎞
0.5𝜎𝑦⎠
⎝
When  tensile  loading  is  applied  after  buckling,  the  member  must  first  be  straightened 
before  the  full  tensile  yield  force  can  be  developed.    This  is  represented  by  a  reduced 
unloading stiffness (e.g.  segment 14-15) and the tensile reloading curve (segments 8-9 
and  15-16).    Further  details  can  be  found  in Bruneau,  Uang,  and Whittaker  [1998]  and 
Structural Engineers Association of California [1974, 1990, 1996]. 
Solid line: λ = 25 (stocky) 
Dashed 
line: 
(slender) 
λ = 120 
Figure M171-2. 
The response of stocky (low λ) and slender (high λ) braces are compared in the graph.  
These  differences  are  achieved  by  altering  the  input  value  LAMDA  (or  the  section 
properties of the beam) and FBUCK.
*MAT_STEEL_CONCENTRIC_BRACE 
Axial Strain and Internal Energy may be plotted from the INTEGRATED beam results 
menus in Oasys Ltd.  Post processors: D3PLOT and T/HIS. 
FEMA thresholds are the total axial strains (defined by change of length/initial length) 
at  which  the  element  is  deemed  to  have  passed  from  one  category  to  the  next,  e.g.  
“Elastic”, “Immediate Occupancy”, “Life Safe”, etc.  During the analysis, the maximum 
tensile  and  compressive  strains  (“high  tide  strains”)  are  recorded.    These  are  checked 
against the user-defined limits TS1 to TS4 and CS1 to CS4.  The output flag is then set to 
0, 1, 2, 3, or 4 according to which limits have been passed.  The value in the output files 
is  the  highest  such  flag  from  tensile  or  compressive  strains.    To  plot  this  data,  select 
INTEGRATED beam results, Integration point 4, Axial Strain. 
Maximum plastic strains in tension and compression are also output.  These are defined 
as maximum total strain to date minus the yield or first buckling strain for tensile and 
compressive  plastic  strains  respectively.    To  plot  these,  select  INTEGRATED  beam 
results,  Integration  point  4,  “shear  stress  XY”  and  “shear  stress  XZ”  for  tensile  and 
compressive plastic strains, respectively.
*MAT_172 
This is Material Type 172, for shell and Hughes-Liu beam elements only.  The material 
model  can  represent  plain  concrete  only,  reinforcing  steel  only,  or  a  smeared 
combination  of  concrete  and  reinforcement.    The  model  includes  concrete  cracking  in 
tension  and  crushing  in  compression,  and  reinforcement  yield,  hardening  and  failure.  
Properties  are  thermally  sensitive;  the  material  model  can  be  used  for  fire  analysis.  
Material data and equations governing the behavior (including thermal properties) are 
taken from Eurocode 2 (EC2).  See notes below for more details of how the standard is 
applied  in  the  material  model.    Although  the  material  model  offers  many  options,  a 
reasonable  response  may  be  obtained  by  entering  only  RO,  FC  and  FT  for  plain 
concrete; if reinforcement is present, YMREINF, SUREINF, FRACRX, FRACRY must be 
defined. Note that, from release R10 onwards, the number of possible cracks has been 
increased from 2 (0 and 90 degrees) to 4 – see notes below. 
NOTE: This material does not support specification of a ma-
terial  angle,  𝛽𝑖,  for  each  through-thickness  integra-
tion point of a shell. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
FC 
F 
4 
FT 
F 
5 
6 
7 
8 
TYPEC 
UNITC 
ECUTEN 
FCC 
F 
F 
F 
F 
Default 
none 
none 
none 
0.0 
1.0 
1.0 
0.0025 
FC 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ESOFT 
LCHAR 
MU 
TAUMXF  TAUMXC  ECRAGG 
AGGSZ 
UNITL 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
See 
notes 
0.0 
0.4 
1020 
1.161 
× FT 
0.001 
0.0 
1.0
Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
YMREINF  PRREINF  SUREINF 
TYPER 
FRACRX 
FRACY 
LCRSU 
LCALPS 
Type 
F 
F 
F 
F 
F 
F 
I 
I 
Default 
none 
0.0 
0.0 
1.0 
0.0 
0.0 
none 
none 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
AOPT 
ET36 
PRT36 
ECUT36 
LCALPC  DEGRAD 
ISHCHK 
UNLFAC 
Type 
F 
F 
F 
F 
I 
F 
Default 
0.0 
0.0 
0.25 
1020 
none 
0.0 
Additional card for AOPT > 0. 
  Card 5 
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
3 
ZP 
F 
4 
A1 
F 
5 
A2 
F 
6 
A3 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
I 
0 
F 
0.5 
7 
8 
Additional card for AOPT > 0. 
  Card 6 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
7 
8 
BETA 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0
Omit if ISHCHK = 0 
  Card 7 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TYPSEC 
P_OR_F 
EFFD 
GAMSC 
ERODET 
ERODEC 
ERODER 
TMPOFF 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
2.0 
0.01 
0.05 
0.0 
Additional card for TYPEC = 6 or 9. 
  Card 8 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ECI_6 
ECSP69  GAMCE9 
PHIEF9 
Type 
F 
F 
F 
F 
Default 
see 
notes 
see 
notes 
0.0 
0.0 
Define this card only if FT is negative. 
  Card 9 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FT2 
FTSHR 
LCFTT  WRO_G 
ZSURF 
Type 
F 
F 
F 
F 
F 
Default  abs(FT)  abs(FT2) 
0.0 
0.0 
0.0
VARIABLE   
DESCRIPTION
MID 
RO 
FC 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Compressive  strength  of  concrete  (stress  units). 
depends on TYPEC. 
  Meaning
TYPEC = 1,2,3,4,5,7,8: FC is the actual compressive strength 
TYPEC = 6: 
TYPEC = 9: 
is 
FC 
strength used in Mander equations.  
the  unconfined  compressive 
FC  is  the  characteristic  compressive 
strength  (fck  in  EC2  1-1).    See  also  FCC 
and the notes below. 
FT 
Tensile stress to cause cracking.  Negative value to read card 9. 
TYPEC 
Concrete 
relationships 
aggregate 
type 
for 
stress-strain-temperature 
EQ.1.0:  Siliceous (default), Draft EC2 Annex (fire engineering)
EQ.2.0:  Calcareous, Draft EC2 Annex (fire engineering) 
EQ.3.0:  Non-thermally-sensitive using ET3, ECU3 
EQ.4.0:  Lightweight 
EQ.5.0:  Fiber-reinforced 
EQ.6.0:  Non-thermally-sensitive, Mander algorithm 
EQ.7.0:  Siliceous, EC2 1-2:2004 (fire engineering) 
EQ.8.0:    Calcareous, EC2 1-2:2004 (fire engineering) 
EQ.9.0:  EC2 1-1:2004 (general and buildings) 
To  obtain  the  pre-R9  behaviour,  i.e.    maximum  of  2  cracks,  add
100  to  TYPEC.    For  example,  109  means  2  cracks,  EC2  1-1:2004 
(general and buildings).
VARIABLE   
UNITC 
DESCRIPTION
Factor  to  convert  stress  units  to  MPa  (used  in  shear  capacity
checks and for application of EC2 formulae when TYPEC = 9) e.g. 
if model units are Newtons and metres, UNITC=10^-6. 
ECUTEN 
Strain to fully open a crack. 
FCC 
Relevant only if TYPEC = 6 or 9. 
TYPEC = 6: 
FCC  is  the  compressive  strength  of  confined 
concrete  used  in  Mander  equations.    Default:  un-
confined properties are assumed. 
TYPEC = 9: 
FCC  is  the  actual  compressive  strength.    If 
blank,  this  will  be  set  equal  to  the  mean  compres-
sive  strength  (fcm  in  EC2  1-1)  as  required  for  ser-
viceability calculations (8MPa greater than FC).  For
ultimate load calculations the user may set FCC to a
factored  characteristic  compressive  strength.    See
notes below. 
ESOFT 
Tension  stiffening  (Slope  of  stress-strain  curve  post-cracking  in 
tension) 
MU 
Friction on crack planes (max shear = 𝜇 × compressive stress) 
TAUMXF 
TAUMXC 
ECRAGG 
AGGSZ 
UNITL 
Maximum  friction  shear  stress  on  crack  planes  (ignored  if 
AGGSZ > 0 - see notes). 
Maximum  through-thickness  shear  stress  after  cracking  . 
Strain parameter for aggregate interlock (ignored if AGGSZ > 0 -
see notes). 
Aggregate size (length units - used in NS3473 aggregate interlock 
formula - see notes). 
Factor  to  convert  length  units  to  millimeters  (used  only  if
AGGSZ > 0 
  if  model  unit  is  meters,
UNITL = 1000. 
  -  see  notes)  e.g. 
LCHAR 
Characteristic length at which ESOFT applies, also  used as  crack
spacing in aggregate-interlock calculation
*MAT_CONCRETE_EC2 
DESCRIPTION
YMREINF 
Young’s Modulus of reinforcement 
PRREINF 
Poisson’s Ratio of reinforcement 
SUREINF 
Ultimate stress of reinforcement 
TYPER 
Type of reinforcement for stress-strain-temperature relationships
EQ.1.0:  Hot rolled reinforcing steel, Draft EC2 Annex (fire) 
EQ.2.0:  Cold  worked  reinforcing  steel  (default),  Draft  EC2
Annex (fire) 
EQ.3.0:  Quenched/tempered  prestressing  steel,  Draft  EC2
Annex (fire) 
EQ.4.0:  Cold worked prestressing steel, Draft EC2 Annex (fire)
EQ.5.0:  Non-thermally sensitive using loadcurve LCRSU. 
EQ.7.0:  Hot rolled reinforcing steel, EC2 1-2:2004 (fire) 
EQ.8.0:  Cold worked reinforcing steel, EC2 1-2:2004 (fire) 
Fraction  of  reinforcement  (𝑥-axis).    For  example,  to  obtain  1% 
reinforcement set FRACR = 0.01. 
Fraction  of  reinforcement  (𝑦-axis).    For  example,  to  obtain  1% 
reinforcement set FRACR = 0.01. 
Loadcurve  for  TYPER = 5,  giving  non-dimensional  factor  on 
SUREINF  versus  plastic 
stress-strain 
relationships from EC2). 
(overrides 
strain 
FRACRX 
FRACRY 
LCRSU 
LCALPS 
Optional  loadcurve  giving  thermal  expansion  coefficient  of
reinforcement vs temperature – overrides relationship from EC2.
VARIABLE   
AOPT 
DESCRIPTION
Material  axes  option  :  
EQ.0.0:  locally  orthotropic  with  material  axes  determined  by 
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES,  and  then  rotated  about  the  shell  ele-
ment normal by an angle BETA. 
EQ.2.0:  globally orthotropic with material axes determined by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0:  locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  𝐯  with  the 
element normal. 
LT.0.0:  This  option  has  not  yet  been  implemented  for  this
material model. 
ET36 
Young’s  Modulus  of  concrete  (TYPEC = 3  and  6).    For  other 
values  of  TYPEC,  the  Young’s  Modulus  is  calculated  internally:
see notes. 
PRT36 
Poisson’s Ratio of concrete (TYPEC = all). 
ECUT36 
Strain to failure of concrete in compression (TYPEC = 3 and 6). 
LCALPC 
DEGRAD 
ISHCHK 
Optional  loadcurve  giving  thermal  expansion  coefficient  of
concrete vs temperature – overrides relationship from EC2. 
If  non-zero,  the  compressive  strength  of  concrete  parallel  to  an
open crack will be reduced . 
Set this flag to 1 to input Card 7 (shear capacity check and other
optional input data). 
UNLFAC 
Stiffness degradation factor after crushing (0.0 to 1.0 – see notes). 
XP, YP, ZP 
Not used. 
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3. 
D1, D2, D3 
Components of vector 𝐝 for AOPT = 2.
BETA 
*MAT_CONCRETE_EC2 
DESCRIPTION
Material  angle  in  degrees  for  AOPT = 0  and  AOPT = 3.    BETA 
may  be  overridden  on  the  element  card,  see  *ELEMENT_-
SHELL_BETA 
TYPESC 
Type of shear capacity check 
EQ.1.0:  BS 8110 
EQ.2.0:  ACI 
P_OR_F 
EFFD 
If BS8110 shear check, percent reinforcement  – e.g.  if 0.5%, input 
0.5.  If ACI shear check, ratio (cylinder strength/FC) - defaults to 
1. 
Effective  section  depth  (length  units),  used  in  shear  capacity
check.    This  is  usually  the  section  depth  excluding  the  cover
concrete. 
GAMSC 
Load factor used in BS8110 shear capacity check. 
ERODET 
Crack-opening strain at which element is deleted 
ERODEC 
Compressive strain used in erosion criteria, see notes 
ERODER 
Reinforcement plastic strain used in erosion criteria, see notes 
TMPOFF 
Constant to be added to the model’s temperature unit to convert
into  degrees  Celsius,  e.g.,  if  the  model’s  temperature  unit  is 
  Degrees  Celsius 
degrees  Kelvin,  set  TMPOFF 
temperatures  are  then  used  throughout  the  material  model,  e.g.,
for  LCALPC  as  well  as  for  the  default  thermally-sensitive 
properties. 
-273. 
to 
EC1_6 
Strain at maximum compressive stress for Type 6 concrete. 
ECSP69 
Spalling strain in compression for TYPEC = 6 and 9. 
GAMCE9 
Material factor that divides the Youngs Modulus (TYPEC = 9). 
PHIEF9 
Effective creep ratio (TYPEC = 9). 
FT2 
Tensile strength used for calculating tensile response. 
FTSHR 
Tensile strength used for calculating post-crack shear response. 
LCFTT 
Loadcurve defining factor on tensile strength versus time.
VARIABLE   
DESCRIPTION
WRO_G 
Density times gravity for water pressure in cracks 
ZSURF 
Z-coordinate of water surface (for water pressure in cracks) 
Remarks: 
reinforced  concrete  with  evenly  distributed 
This material model can be used to represent unreinforced concrete (FRACR = 0), steel 
(FRACR = 1),  or 
reinforcement 
(0 < FRACR < 1).    Concrete  is  modelled  as  an  initially-isotropic  material  with  a  non-
rotating  smeared  crack  approach  in  tension,  together  with  a  plasticity  model  for 
compressive  loading.    Reinforcement  is  treated  as  separate  sets  of  bars  in  the  local 
element  x  and  y  axes.    The  reinforcement  is  assumed  not  to  carry  through-thickness 
shear  or  in-plane  shear.    Therefore,  this  material  model  should  not  be  used  to  model 
steel-only sections, i.e.  do not create a section in which all the integration points are of 
*MAT_172 with FRACRX, FRACRY = 1.  
Creating Reinforced Concrete Sections: 
Reinforced concrete sections for shell or beam elements may  be created using *PART_
COMPOSITE  (for  shells)  or  *INTEGRATION_BEAM  (for  beams)  to  define  the  section.  
Create one Material definition representing the concrete using MAT_CONCRETE_EC2 
with  FRACR = 0.    Create  another  Material  definition  representing  the  reinforcement 
using MAT_CONCRETE_EC2 with FRACRX and/or FRACRY = 1.  The Material ID of 
each  integration  point  is  then  set  to represent  either  concrete  or  steel.    The  position  of 
each integration point within the cross-section and its cross-sectional area are chosen to 
represent the actual distribution of reinforcement.  
Options for TYPEC and TYPER 
Eurocode  2  (EC2)  contains  different  sections  applicable  to  general  structural 
engineering  versus  fire  engineering.    The  latter  contains  different  data  for  different 
types of concrete and steel, and has been revised during its history.  TYPEC and TYPER 
control  the  version  and  section  of  the  EC2  document  from  which  the  material  data  is 
taken,  and  the  types  of  concrete  and  steel  being  represented.    In  the  descriptions  of 
TYPEC and TYPER above, “Draft EC2 Annex (fire engineering)” means data taken from 
the 1995 draft Eurocode 2 Part 1-2 (for fire engineering), ENV 1992-1-2:1995.  These are 
the  defaults,  and  are  suitable  for  general  use  where  elevated  temperatures  are  not 
considered. 
EC2 was then issued in 2004 (described above as EC2 1-2:2004 (fire)) with revised stress-
strain  data  at  elevated  temperatures  (TYPEC  and  TYPER = 7  or  8).    These  settings  are 
recommended for analyses with elevated temperatures.
Meanwhile  Eurocode  2  Part  1-1  (for  general  structural  engineering),  EC2  1-1:2004, 
contains  material  data  and  formulae  that  differ  from  Part  1-2;  these  are  obtained  by 
setting TYPEC = 9.  This setting is recommended where compatibility is required with 
the structural engineering data and assumptions of Part 1-1 of the Eurocode. 
A  further  option  for  modelling  concrete,  TYPEC = 6,  is  provided  for  applications  such 
as seismic engineering in which the different stress-strain behaviors of confined versus 
unconfined concrete needs to be captured.  This option uses equations by Mander et al, 
and does not relate directly to Eurocode 2.  
Material Behavior: Concrete 
Thermal sensitivity 
For  TYPEC = 1,2,4,5,7,8,  the  material  properties  are  thermally-sensitive. 
  If  no 
temperatures  are  defined  in  the  model,  it  behaves  as  if  at  20degC.    Pre-programmed 
relationships  between  temperature  and  concrete  properties  are  taken  from  the  EC2 
document.    The  thermal  expansion  coefficient  is  as  defined  in  EC2,  is  non-zero  by 
default,  and  is  a  function  of  temperature.    This  may  be  overridden  by  inputting  the 
curve  LCALPC.    TYPEC = 3,  6  and  9  are  not  thermally  sensitive  and  have  no  thermal 
expansion coefficient by default. 
Tensile response 
The  concrete  is  assumed  to  crack  in  tension  when  the  maximum  in-plane  principal 
stress  reaches  FT.    A  non-rotating  smeared  crack  approach  is  used.    Cracks  can  open 
and  close  repeatedly  under  hysteretic  loading.    When  a  crack  is  closed  it  can  carry 
compression  according  to  the  normal  compressive  stress-strain  relationships.    The 
direction of the crack relative to the element coordinate system is stored when the crack 
first  forms.    The  material  can  carry  compression  parallel  to  the  crack  even  when  the 
crack is open. Further cracks may then form at pre-determined angles to the first crack, 
if the tensile stress in that direction reaches FT.  In versions up to R9.0, the number of 
further cracks is limited to one, at 90 degrees to the first crack.  In versions starting from 
R10,  up  to  three  further  cracks  can  form,  at  45,  90  amd  135  degrees  to  the  first  crack.  
The  tensile  stress  is  limited  to  FT  only  in  the  available  crack  directions.    The  tensile 
stress in other directions is unlimited, and could exceed FT.  This is a limitation of the 
non-rotating  crack  approach  and  may  lead  to  models  being  non-conservative,  i.e.    the 
response is stronger than implied by the input.  The increase of the possible number of 
cracks from two to four significantly reduces this error, and may therefore cause models 
to seem “weaker” in R10 than in R9 under some loading conditions.  An option to revert 
to the previous 2-crack behaviour is available in R10 – add 100 to TYPEC.
After  initial  cracking,  the  tensile  stress  reduces  with  increasing  tensile  strain.    A  finite 
amount  of  energy  must  be  absorbed  to  create  a  fully  open  crack  -  in  practice  the 
reinforcement holds the concrete together, allowing it to continue to take some tension 
(this  effect  is  known  as  tension-stiffening).    The  options  available  for  the  stress-strain 
relationship are shown below.  The bilinear relationship is used by default.  The simple 
linear relationship applies only if ESOFT > 0 and ECUTEN = 0. 
Figure M172-1.  Tensile Behaviour of Concrete 
LCHAR  can  optionally  be  used  to  maintain  constant  energy  per  unit  area  of  crack 
irrespective  of  mesh  size,  i.e.    the  crack  opening  displacement  is  fixed  rather  than  the 
crack  opening  strain.    LCHAR ×  ECUTEN  is  then  the  displacement  to  fully  open  a 
crack.    For  the  actual  elements,  crack  opening  displacement  is  estimated  by  strain ×
√area.  Note that if LCHAR is defined, it is also used as the crack spacing in the NS 3473 
aggregate interlock calculation. 
For the thermally-sensitive values of TYPEC, the relationship of FT with temperature is 
taken from EC2 – there is no input option to change this.  FT is assumed to remain at its 
input  value  at  temperatures  up  to  100°C,  then  to  reduce  linearly  with  temperature  to 
zero  at  600°C.    Up  to  500°C,  the  crack  opening  strain  ECUTEN  increases  with 
temperature  such  that  the  fracture  energy to  open  the  crack  remains  constant.    Above 
500 deg C the crack opening strain does not increase further. 
In some concrete design codes and standards, it is stipulated that the tensile strength of 
concrete should be assumed to be zero.  However, for MAT_CONCRETE_EC2 it is not 
recommended to set FT to zero, because: 
•Cracks will form at random orientations caused by small dynamic tensile stresses, 
leading  to  unexpected  behavior  when  the  loading  increases  because  the  crack 
orientations are fixed when the cracks first form;  
•The  shear  strength of cracked  concrete  may then  also  become  zero  in  the  analysis 
(according  to  the  aggregate  interlock  formula,  the  post-crack  shear  strength  is 
assumed proportional to FT).
These problems may be tackled by using the inputs on Card 9.  Firstly, separate tensile 
strengths may be input for the tensile response and for calculating the shear strength of 
cracked concrete.  Secondly, by using the loadcurve LCFTT, the tensile strength may be 
ramped gradually down to zero after the static loads have been applied, ensuring that 
the cracks will form in the correct orientation 
Compressive response: TYPEC = 1,2,4,5,7,8 
For  TYPEC = 1,2,4,5,7,8,  the  compressive  behavior  of  the  concrete  initially  follows  a 
stress-strain curve defined in EC2 as: 
Stress = FCmax ×
) ×
𝜀cl
⎡(
⎢
⎣
2 + ( 𝜀
𝜀cl
)
⎤ 
⎥
⎦
where 𝜀cl is the strain at which the ultimate compressive strength FCmax is reached, and 
𝜀 is the current equivalent uniaxial compressive strain. 
The initial elastic modulus is given by 𝐸 = 3 × FCmax/2𝜀cl. On reaching FCmax, the stress 
decreases linearly with increasing strain, reaching zero at a strain 𝜀cu. Strains 𝜀cl and 𝜀cu 
are  by  default  taken  from  EC2  and  are  functions  of  temperature.    At  20oC  they  take 
values  0.0025  and  0.02  respectively.  FCmax  is  also  a  function  of  temperature,  given  by 
the  input  parameter  FC  (which  applies  at  20oC)  times  a  temperature-dependent 
softening  factor  taken  from  EC2.    The  differences  between  TYPEC = 1,2,4,5,7,8  are 
limited  to  (a)  different  reductions  of  FC  at  elevated  temperatures,  and  (b)  different 
values of 𝜀cl at elevated temperatures. 
Figure M172-2.  Concrete stress strain behavior 
Compressive response: TYPEC = 3
For  TYPEC = 3,  the  user  over-rides  the  default  values  of  Young’s  Modulus  and  𝜀cu  
using ET36 and ECUT36 respectively.  In this case, the strain 𝜀cl is calculated from the 
elastic stiffness, and there is no thermal sensitivity.  The stress-strain behaviour follows 
the same form as described above. 
Compressive response: TYPEC = 6 
For  TYPEC = 6,  the  above  compressive  crushing  behaviour  is  replaced  with  the 
equations  proposed  by  Mander.    This  algorithm  can  model  unconfined  or  confined 
concrete;  for  unconfined,  leave  FCC  blank.    For  confined  concrete,  input  the  confined 
compressive strength as FCC.  
Figure M172-3.  Type 6 concrete 
Default values for type 6 are calculated as follows: 
𝜀cl = 0.002 × [1 + 5 (
FCC6
FC
− 1)] 
𝜀cu = 1.1 × 𝜀c 
𝜀csp = 𝜀cu + 2
FCC
Note that for unconfined concrete, FCC6 = FC causing 𝜀cl to default to 0.002. 
Compressive response: TYPEC = 9
For  TYPEC = 9,  the  input  parameter  FC  is  the  characteristic  cylinder  strength  in  the 
stress units of the  model.  FC x UNITC is assumed to be fck, the  strength class in MPa 
units.  The mean tensile strength fctm, mean Young’s Modulus Ecm, and the strains used 
to  construct  the  stress-strain  curve  such  as  𝜀cl  are  by  default  evaluated  automatically 
from tabulated functions of fck given in Table 3.1 of EC2.  The compressive strength of 
the  material  is  given  by  the  input  parameter  FCC,  which  defaults  to  the  mean 
compressive  strength  fcm  defined  in  EC2  as  fck  +  8MPa).    The  user  may  override  the 
default  compressive  strength  by  inputting  FCC  explicitly.    The  stress-strain  curve 
follows this form: 
𝑆𝑡𝑟𝑒𝑠𝑠
𝐹𝐶𝐶
=  
𝑘𝜂 −   𝜂2
1 + (𝑘 − 2)𝜂
Where FCC is the input parameter FCC (default: = (fck + 8MPa)/UNITC), 
𝜼 = 𝒔𝒕𝒓𝒂𝒊𝒏/𝜺cl, 
𝒌 = 𝟏. 𝟎𝟓𝑬 ×  
𝜺𝒄𝟏
𝑭𝑪𝑪⁄
E is the Young’s Modulus.  
The  default  parameters  are  intended  to  be  appropriate  for  a  serviceability  analysis 
(mean  properties),  so  default  FT = fctm  and  default  E = Ecm.    For  an  ultimate  load 
analysis,  FCC  should  be  the  “design  compressive  strength”  (normally  the  factored 
characteristic strength, including any appropriate material factors); FT should be input 
as the factored characteristic tensile strength; GAMCE9 may be input (a material factor 
that  divides  the  Young’s  Modulus  so  E = Ecm/GAMCE9);  and  a  creep  factor  PHIEF9 
may be input: this scales 𝜺cl  by (1+PHIEF9).  
Unload/reload stiffness (all concrete types): 
During  compressive  loading,  the  elastic  modulus  will  be  reduced  according  to  the 
parameter UNLFAC (default = 0.5).  UNLFAC = 0.0 means no reduction, i.e.  the initial 
elastic modulus will apply during unloading and reloading.  UNLFAC = 1.0 means that 
unloading  results  in  no  permanent  strain.    Intermediate  values  imply  a  permanent 
strain linearly interpolated between these extremes.
Figure M172-4.  Concrete unloading behavior 
Tensile  strength is reduced by the same factor as the elastic modulus as described in the 
paragraph above. 
Optional compressive strength degradation due to cracking: 
By default, the compressive strength of cracked and uncracked elements is the same.  If 
DEGRAD is non-zero, the formula from BS8110 is used to reduce compressive strength 
parallel to the crack while the crack is open: 
Reduction factor = min (1.0,
1.0
0.8 + 100𝜀𝑡
) , 
where 𝜀𝑡 is the tensile strain normal to the crack. 
Shear strength on crack planes: 
Before  cracking,  the  through-thickness  shear  stress  in  the  concrete  is  unlimited.    For 
cracked elements, shear stress on the crack plane (magnitude of shear stress including 
element-plane and through-thickness terms) is treated in one of two ways: 
1. 
If  AGGSZ > 0,  the  relationship  from  Norwegian  standard  NS3473  is  used  to 
model the aggregate-interlock that allows cracked concrete to carry shear load-
ing.  In this case, UNITL must be defined.  This is the factor that converts model 
length  units  to  millimetres,  i.e.    the  aggregate  size  in  millimetres = AGGSZ × 
UNITL.    The  formula  in  NS3473  also  requires  the  crack  width  in  millimetres: 
this  is  estimated  from  UNITL × 𝜀cro × 𝐿𝑒,  here  𝜀cro  is  the  crack  opening  strain 
and  𝐿𝑒  is  the  crack  spacing,  taken  as  LCHAR  if  non-zero,  or  equal  to  element 
size if LCHAR is zero.  Optionally, TAUMXC may be used to set the maximum 
shear stress when the crack is closed and the normal stress is zero – by default
this is equal to 1.161FT from the formulae in NS3473.  If TAUMXC is defined, 
the shear stress from the NS3473 formula is scaled by TAUMXC / 1.161FT. 
2. 
If AGGSZ = 0, the aggregate interlock is modeled by this formula: 
𝜏max =
TAUMXC
𝜀cro
ECRAGG
1.0 +
+ min(MU × 𝜎comp,TAUMXF) 
Where  𝜏max  is  the  maximum  shear  stress  carried  across  a  crack;  𝜎compis  the 
compressive stress across the crack (this is zero if the crack is open); ECRAGG 
is  the  crack  opening  strain  at  which  the  input  shear  strength  TAUMXC  is 
halved.  Again, TAUMXC defaults to 1.161FT. 
Note that if a shear capacity check is specified, the above applies only to in-plane shear, 
while the through-thickness shear is unlimited. 
Reinforcement 
The  reinforcement  is  treated  as  separate  bars  providing  resistance  only  in  the  local  𝑥 
and 𝑦 directions – it does not carry shear in-plane or out of plane.  
For  TYPER = 1,2,3,4,7,8,  the  behaviour  is  thermally  sensitive  and  follows  stress-strain 
relationships of a form defined in EC2.  At 20oC (or if no thermal input is defined) the 
behaviour is elastic-perfectly-plastic with Young’s Modulus EREINF and ultimate stress 
SUREINF,  up  to  the  onset  of  failure,  after  which  the  stress  reduces  linearly  with 
increasing  strain  until  final  failure.    At  elevated  temperatures  there  is  a  nonlinear 
transition  between  the  elastic  phase  and  the  perfectly  plastic  phase,  and  EREINF  and 
SUREINF  are  scaled  down  by  temperature-dependent  factors  defined  in  EC2.    The 
strain  at  which  failure  occurs  depends  on  the  reinforcement  type  (TYPER)  and  the 
temperature.  For example, for hot-rolled reinforcing steel at 20oC failure begins at 15% 
strain and is complete at 20% strain. The thermal expansion coefficient is as defined in 
EC2 and is a function of temperature.  This may be overridden by inputting the curve 
LCAPLS.    The  differences  between  TYPER = 1,2,4,7,8  are  limited  to  (a)  different 
reductions  of  EREINF  and  SUREINF  at  elevated  temperatures,  (b)  different  nonlinear 
transitions  between  elastic  and  plastic  phases  and  (c)  the  strains  at  which  softening 
begins and is complete. 
The  default  stress-strain  curve  for  reinforcement  may  be  overridden  using  TYPER = 5 
and  LCRSU.    In  this  case,  the  reinforcement  properties  are  not  temperature-sensitive 
and the yield stress is given by SUREINF × 𝑓 (𝜀𝑝), where 𝑓 (𝜀𝑝) is the loadcurve value at 
the  current  plastic  strain.    To  include  failure  of  the  reinforcement,  the  curve  should 
reduce to zero at the desired failure strain and remain zero for higher strains.  Note that 
by default LS-DYNA re-interpolates the input curve to have 100 equally-spaced points;
if the last point on the curve is at very high strain, then the initial part of the curve may 
become poorly defined. 
Local directions: 
AOPT and associated data are used to define the directions of the reinforcement bars.  If 
the  reinforcement  directions  are  not  consistent  across  neighbouring  elements,  the 
response may be less stiff than intended – this is equivalent to the bars being bent at the 
element boundaries.  See material type 2 for description of the different AOPT settings. 
Shear capacity check: 
Shear reinforcement is not included explicitly in this material model.  However, a shear 
capacity  check  can  be  made,  to  show  regions  that  require  shear  reinforcement.    The 
assumption  is  that  the  structure  will  not  yield  or  fail  in  through-thickness  shear, 
because  sufficient  shear  reinforcement  will  be  added.    Set  ISHCHK  and  TYPESC  to  1.  
Give  the  percentage  reinforcement  (P_OR_F),  effective  depth  of  section  EFFD  (this 
typically excludes the cover concrete), and load factor GAMSC.  These are used in Table 
3.8 of BS 8110-1:1997 to determine the design shear stress.  The “shear capacity” is this 
design shear stress times the total section thickness (i.e.  force per unit width), modified 
according to Equation 6b of BS 8110 to allow for axial load.  The “shear demand” (actual 
shear  force  per  unit  width)  is  then  compared  to  the  shear  capacity.    This  process  is 
performed  for  the  two  local  directions  of  the  reinforcement  in  each  element;  when 
defining  sections  using  integration  rules  and  multiple  sets  of  material  properties,  it  is 
important that each set of material properties referenced within the same section has the 
same AOPT and orientation data.  Note that the shear demand and axial load (used in 
calculation  of  the  shear  capacity)  are  summed  across  the  integration  points  within  the 
section;  the  same  values  of  capacity,  demand,  and  difference  between  capacity  and 
demand are then written to all the integration points.
*MAT_CONCRETE_EC2 
By  default,  thermal  expansion  properties  from  EC2  are  used.    If  no  temperatures  are 
defined  in  the  model,  properties  for  20deg  C  are  used.    For  TYPEC = 3,  6  or  9,  and 
TYPER = 5,  there  is  no  thermal  expansion  by  default,  and  the  properties  do  not  vary 
with temperature.  The user may override the default thermal expansion behaviour by 
defining  curves  of  thermal  expansion  coefficient  versus  temperature  (LCALPC, 
LCALPR).  These apply no matter what types TYPEC and TYPER have been selected. 
Output: 
“Plastic  Strain”  is  the  maximum  of  the  plastic  strains  in  the  reinforcement  in  the  two 
local directions. 
Element deletion: 
Elements  are  deleted  from  the  calculation  when  all  of  their  integration  points  have 
reached the erosion criterion: 
Concrete crack opening strain > ERODET 
           or Concrete compressive strain > εc_erode 
where εc_erode = ERODEC + εcsp with εcsp the strain at which the stress-strain relation falls 
to zero. 
Reinforcement plastic strain > εr_erode 
where = ERODER  +  εrsp  with  εrsp  the  strain  at  which  the  stress-strain  relation  falls  to 
zero, or if LCRSU > 0 εrsp is assumed to be 2.0. 
If the material is smeared concrete/reinforcement, i.e.  0 < max(FRACRX, FRACRY) < 1, 
the erosion criteria must be met for both concrete and reinforcement before erosion can 
occur 
Extra  history  variables  may  be  requested  for  shell  elements  (NEIPS  on  *DATABASE_-
EXTENT_BINARY), which have the following meaning: 
Extra Variable  1:  Current  crack  opening  strain  (if  two  cracks  are  present,  max 
of the two) 
Extra Variable  2:  Equivalent  uniaxial 
strain 
for 
concrete 
compressive 
behaviour 
Extra Variable  3:  Number of cracks (0, 1 or 2)
Extra Variable  4:  Temperature 
Extra Variable  5:  Thermal strain 
Extra Variable  6:  Current crack opening strain – first crack to form 
Extra Variable  7:  Current  crack  opening  strain  –  crack  at  90  degrees  to  first 
crack  
Extra Variable  8:  Max crack opening strain – first crack to form  
Extra Variable  9:  Max crack opening strain – crack at 90 degrees to first crack  
Extra Variable  10:  Maximum difference (shear demand minus capacity) that has 
occurred so far, in either of the two reinforcement directions 
Extra Variable  11:  Maximum difference (shear demand minus capacity) that has 
occurred so far, in reinforcement 𝑥-direction  
Extra Variable  12:  Maximum difference (shear demand minus capacity) that has 
occurred so far, in reinforcement 𝑦-direction  
Extra Variable  13:  Current  shear  demand  minus  capacity,  in  reinforcement  𝑥-
direction  
Extra Variable  14:  Current  shear  demand  minus  capacity,  in  reinforcement  𝑦-
direction  
Extra Variable  15:  Current shear capacity 𝑉cx, in reinforcement 𝑥-direction  
Extra Variable  16:  Current shear capacity 𝑉cy, in reinforcement 𝑦-direction  
Extra Variable  17:  Current shear demand 𝑉x, in reinforcement 𝑥-direction  
Extra Variable  18:  Current shear demand 𝑉y, in reinforcement 𝑦-direction  
Extra Variable  19:  Maximum  shear  demand  that  has  occurred  so  far,  in 
reinforcement x-direction  
Extra Variable  20:  Maximum  shear  demand)  that  has  occurred  so  far,  in 
reinforcement y-direction  
Extra Variable  21:  Current strain in reinforcement (𝑥-direction) 
Extra Variable  22:  Current strain in reinforcement (𝑦-direction) 
Extra Variable  23:  Engineering shear strain (slip) across first crack  
Extra Variable  24:  Engineering shear strain (slip) across second crack  
Extra Variable  25:  𝑥-stress in concrete (element local axes) 
Extra Variable  26:  𝑦-stress in concrete (element local axes) 
Extra Variable  27:  𝑥𝑦-stress in concrete (element local axes) 
Extra Variable  28:  𝑦𝑧-stress in concrete (element local axes) 
Extra Variable  29:  𝑥𝑧-Stress in concrete (element local axes)
Extra Variable  30:  Reinforcement stress (𝑎-direction) 
Extra Variable  31:  Reinforcement stress (𝑏-direction) 
Extra Variable  32:  Current shear demand 𝑉max 
Extra Variable  33:  Maximum 𝑉max that has occurred so far 
Extra Variable  34:  Current shear capacity 𝑉cθ 
Extra Variable  35:  Excess shear: 𝑉max − 𝑉cθ 
Extra Variable  36:  Maximum excess shear that has occurred so far 
In the above list 𝑉max is given by 
𝑉max = √𝑉𝑥
2 
2 + 𝑉𝑦
Where 𝑉𝑥 and 𝑉𝑦 is the shear demand reinforcement in 𝑥 and 𝑦 directions respectively.  
Additionally, 
𝑉𝑐𝜃 =
√
√√
⎷
𝑉max
)
(
𝑉𝑥
𝑉𝑐𝑥
+ (
𝑉𝑦
𝑉𝑐𝑦
)
where 𝑉𝑐𝑥, 𝑉𝑐𝑦 are the shear capacities in the 𝑥 and 𝑦 directions. 
Note  that  the  concrete  stress  history  variables  are  stored  in  element  local  axes 
irrespective  of  AOPT,  i.e.    local  𝑥  is  always  the  direction  from  node  1  to  node  2.    The 
reinforcement  stresses  are  in  the  reinforcement  directions;  these  do  take  account  of 
AOPT. 
MAXINT (shells) and/or BEAMIP (beams) on *DATABASE_EXTENT_BINARY may be 
set  to  the  maximum  number  of  integration  points,  so  that  results  for  all  integration 
points can be plotted separately.
*MAT_173 
This  is  Material  Type  173  for  solid  elements only,  is  intended  to represent  sandy  soils 
and other granular materials.  Joints (planes of weakness) may be added if required; the 
material then represents rock.  The joint treatment is identical to that of *MAT_JOINT-
ED_ROCK. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
RO 
GMOD 
RNU 
(blank) 
PHI 
CVAL 
PSI 
Type 
A8 
F 
F 
F 
F 
F 
F 
Default 
0.0 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NOVOID  NPLANES 
(blank) 
LCCPDR 
LCCPT 
LCCJDR 
LCCJT 
LCSFAC 
Type 
Default 
1 
0 
  Card 3 
1 
I 
0 
2 
3 
I 
0 
4 
I 
0 
5 
I 
0 
6 
I 
0 
7 
I 
0 
8 
Variable  GMODDP  GMODGR  LCGMEP 
LCPHIEP 
LCPSIEP 
LCGMST  CVALGR 
ANISO 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
1.0
Plane Cards.  Repeat for each plane (maximum 6 planes). 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DIP 
DIPANG 
CPLANE  FRPLANE
TPLANE  SHRMAX 
LOCAL 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
1.e20 
0.0 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density 
GMOD 
Elastic shear modulus 
RNU 
PHI 
Poisson’s ratio 
Angle of friction (radians) 
CVAL 
Cohesion value (shear strength at zero normal stress) 
PSI 
Dilation angle (radians) 
NOVOID 
Flag = 1 to switch off voiding behavior  
NPLANES 
Number of joint planes (maximum 6) 
LCCPDR 
Load  curve  for  extra  cohesion  for  parent  material  (dynamic
relaxation) 
LCCPT 
Load curve for extra cohesion for parent material (transient) 
LCCJDR 
Load curve for extra cohesion for joints (dynamic relaxation) 
LCCJT 
Load curve for extra cohesion for joints (transient) 
LCSFAC 
Load curve giving factor on strength vs.  time 
GMODDP 
Z-coordinate  at which GMOD and CVAL are correct 
GMODGR 
Gradient of GMOD versus z-coordinate (usually negative)
VARIABLE   
DESCRIPTION
LCGMEP 
Load curve of GMOD versus plastic strain (overrides GMODGR) 
LCPHIEP 
Load curve of PHI versus plastic strain 
LCPSIEP 
Load curve of PSI versus plastic strain 
LCGMST 
(Leave blank) 
CVALGR 
Gradient of CVAL versus z-coordinate (usually negative) 
ANISO 
Factor  applied  to  elastic  shear  stiffness  in  global  XZ  and  YZ 
planes 
DIP 
Angle of the plane in degrees below the horizontal 
DIPANG 
Plan view angle (degrees) of downhill vector drawn on the plane 
CPLANE 
Cohesion for shear behavior on plane 
PHPLANE 
Friction angle for shear behavior on plane (degrees) 
TPLANE 
Tensile strength across plane (generally zero or very small) 
SHRMAX 
Max  shear  stress  on  plane  (upper 
compression) 
limit, 
independent  of
LOCAL 
EQ.0: DIP and DIPANG are with respect to the global axes 
EQ.1: DIP  and  DIPANG  are  with  respect  to  the  local  element 
axes 
Remarks: 
1.  The material has a Mohr Coulomb yield surface, given by τmax = C + σntan(PHI), 
where  τmax = maximum  shear  stress  on  any  plane,  σn =  normal  stress  on  that 
plane (positive in compression), C = cohesion, PHI = friction angle.  The plastic 
potential function is of the form βσk - σI + constant, where σk = maximum prin-
cipal stress, σi = minimum principal stress, and 𝛽 = 1+sin(PSI)
1−sin(PSI). 
2.  The  tensile  strength  of  the  material  is  given  by  𝜎max = 𝐶
tan(PHI)  where  C  is  the 
cohesion.  After the material reaches its tensile strength, further tensile straining 
leads to volumetric voiding; the voiding is reversible if the strain is reversed.
3. 
If depth-dependent properties are used, the model must be oriented with the z-
axis in the upward direction. 
4.  Plastic strain is defined as √2
3 𝜀𝑝𝑖𝑗𝜀𝑝𝑖𝑗, i.e.  the same way as for other elasto-plastic 
material models. 
5.  Friction and dilation angles PHI and PSI may vary with plastic strain, to model 
heavily consolidated materials under large shear strains – as the strain increas-
es, the dilation angle typically reduces to zero and the friction angle to a lower, 
pre-consolidation value. 
6.  For similar reasons, the shear modulus may reduce with plastic strain, but this 
option may sometimes give unstable results. 
7.  The  loadcurves  LCCPDR,  LCCPT,  LCCJDR,  LCCJT  allow  extra  cohesion  to  be 
specified  as  a  function  of  time.    The  cohesion  is  additional  to  that  specified  in 
the material parameters.  This is intended for use during the initial stages of an 
analysis to allow application of gravity or other loads without cracking or yield-
ing, and for the cracking or yielding then to be introduced in a controlled man-
ner.    This  is  done  by  specifying  extra  cohesion  that  exceeds  the  expected 
stresses  initially,  then  declining  to  zero.    If  no  curves  are  specified,  no  extra 
cohesion is applied. 
8.  The loadcurve for factor on strength applies simultaneously to the cohesion and 
tan(friction angle) of parent material and all joints.  This feature is intended for 
reducing the strength of the material gradually, to explore factors of safety.  If 
no curve is present, a constant factor of 1 is assumed.  Values much greater than 
1.0 may cause problems with stability. 
9.  The anisotropic factor ANISO applies the elastic shear stiffness in the global XZ 
  It  can  be  used  only  in  pure  Mohr-Coulomb  mode 
and  YZ  planes. 
(NPLANES = 0). 
10.  For friction angle greater than zero, the Mohr Coulomb yield surface implies a 
tensile  pressure  limit  equal  to  CVAL/tan(PHI).    The  default  behaviour  is  that 
voids develop in the material when this pressure limit is reached, and the pres-
sure  will  never  become  more  tensile  than  the  pressure  limit.    If  NOVOID = 1, 
the  tensile  pressure  limit  is  not  applied.   Stress  states  in  which  the  pressure  is 
more tensile than CVAL/tan(PHI) are permitted, but will be purely hydrostatic 
with no shear stress.  NOVOID is recommended in Multi-Material ALE simula-
tions, in which the development of voids or air space is already accounted for 
by the Multi-Material ALE. 
11.  To  model  soil,  set  NJOINT = 0.    The  joints  are  to  allow  modeling  of  rock,  and 
are treated identically to those of *MAT_JOINTED_ROCK.
12.  The  joint  plane  orientations  are  defined  by  the  angle  of  a  “downhill  vector” 
drawn  on  the  plane,  i.e.    the  vector  is  oriented  within  the  plane  to  obtain  the 
maximum possible downhill angle.  DIP is the angle of this line below the hori-
zontal.  DIPANG is the plan-view angle of the line (pointing down hill) meas-
ured clockwise from the global Y-axis about the global Z-axis. 
13.  Joint  planes  would  generally  be  defined  in  the  global  axis  system  if  they  are 
taken from survey data.  However, the material model can also be used to rep-
resent  masonry,  in  which  case  the  weak  planes  represent  the  cement  and  lie 
parallel to the local element axes. 
14.  The joint planes rotate with the rigid body motion of the elements, irrespective 
of whether their initial definitions are in the global or local axis system. 
15.  Extra  variables  for  plotting.    By  setting  NEIPH  on  *DATABASE_EXTENT_BI-
NARY to 27, the following variables can be plotted in Oasys Ltd.  Post Proces-
sors D3PLOT, T/HIS and LS-PrePost: 
Variable(s) 
Description 
1 
2 
3 
4 – 9 
10 - 15 
16 - 20 
21 - 27 
33 
34 
mobilized strength fraction for base material 
volumetric void strain 
maximum stress overshoot during plastic calculation 
crack opening strain for planes 1 - 6 
crack accumulated engineering shear strain for planes 1 - 6 
current shear utilization for planes 1 - 6 
maximum shear utilization to date for planes 1 – 6 
elastic shear modulus (for checking depth-dependent input) 
cohesion (for checking depth-dependent input)
*MAT_RC_BEAM 
This is Material Type 174, for Hughes-Liu beam elements only.  The material model can 
represent  plain  concrete  only,  reinforcing  steel  only,  or  a  smeared  combination  of 
concrete  and  reinforcement.    The  main  emphasis  of  this  material  model  is  the  cyclic 
behavior – it is intended primarily for seismic analysis. 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
EUNL 
Type 
A8 
F 
F 
4 
PR 
F 
5 
FC 
F 
6 
7 
8 
EC1 
EC50 
RESID 
F 
F 
F 
Default 
none 
none 
See 
Remarks 
0.0 
none 
0.0022 
See 
Remarks 
0.2 
  Card 2 
Variable 
1 
FT 
2 
3 
4 
5 
6 
7 
8 
UNITC 
(blank) 
(blank) 
(blank) 
ESOFT 
LCHAR 
OUTPUT 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
See 
Remarks 
1.0 
none 
none 
none 
See 
Remarks 
none 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
F 
0 
8 
Variable 
FRACR 
YMREIN 
PRREIN 
SYREIN 
SUREIN 
ESHR 
EUR 
RREINF 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
none 
0.0 
0.0 
SYREIN
0.03 
0.2 
4.0 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified.
VARIABLE   
DESCRIPTION
RO 
Mass density 
EUNL 
Initial unloading elastic modulus . 
PR 
FC 
EC1 
EC50 
Poisson’s ratio. 
Cylinder strength (stress units) 
Strain at which stress FC is reached. 
Strain at which the stress has dropped to 50% FC 
RESID 
Residual strength factor 
FT 
Maximum tensile stress 
UNITC 
Factor to convert stress units to MPa  
ESOFT 
Slope of stress-strain curve post-cracking in tension 
LCHAR 
Characteristic length for strain-softening behavior 
OUTPUT 
Output flag controlling what is written as “plastic strain” 
EQ.0.0: Curvature 
EQ.1.0: “High-tide” plastic strain in reinforcement 
FRACR 
Fraction  of 
FRACR = 0.01) 
reinforcement 
(e.g. 
for  1% 
reinforcement
YMREIN 
Young’s Modulus of reinforcement 
PRREIN 
Poisson’s Ratio of reinforcement 
SYREIN 
Yield stress of reinforcement 
SUREIN 
Ultimate stress of reinforcement 
ESHR 
EUR 
R_REINF 
Strain at which reinforcement begins to harden 
Strain at which reinforcement reaches ultimate stress 
Dimensionless  Ramberg-Osgood  parameter  r.    If  zero,  a  default 
value  r = 4.0  will  be  used.    If  set  to  -1,  parameters  will  be 
calculated from Kent & Park formulae.
Creating sections for reinforced concrete beams: 
This material model can be used to represent unreinforced concrete (FRACR = 0), steel 
reinforcement 
(FRACR = 1),  or 
(0 < FRACR < 1). 
reinforced  concrete  with  evenly  distributed 
Alternatively,  use  *INTEGRATION_BEAM  to  define  the  section.    A  new  option  in 
allows  the  user  to  define  a  Part  ID  for  each  integration  point,  similar  to  the  facility 
already  available  with  *INTEGRATION_SHELL.    All  parts  referred  to  by  one 
integration  rule  must  have  the  same  material  type,  but  can  have  different  material 
properties.    Create  one  Part  for  concrete,  and  another  for  steel.    These  Parts  should 
reference Materials, both of type *MAT_RC_BEAM, one with FRACR = 0, the other with 
FRACR = 1.  Then, by assigning one or other of these Part Ids to each integration point 
the reinforcement can be applied to the correct locations within the section of the beam. 
Concrete: 
In  monotonic  compression,  the  approach  of  Park  and  Kent,  as  described  in  Park  & 
Paulay  [1975]  is  used.    The  material  follows  a  parabolic  stress-strain  curve  up  to  a 
maximum stress equal to the cylinder strength FC; therafter the strength decays linearly 
with  strain  until  the  residual  strength  is  reached.    Default  values  for  some  material 
parameters will be calculated automatically as follows: 
EC50 =
(3 + 0.29𝐹𝐶)
145𝐹𝐶 − 1000
where FC is in MPa as per Park and Kent test data. 
EUNL  =  initial tangent slope  =
2FC
EC1
User-defined values for EUNL lower than this are not permitted, but higher values may 
be defined  if desired. 
FT = 1.4 (
FC
10
)
where FC is in MPa as per Park and Kent test data. 
ESOFT = EUNL 
User-defined values higher than EUNL are not permitted. 
UNITC is used only to calculate default values for the above parameters from FC. 
Strain-softening  behavior  tends  to  lead  to  deformations  being  concentrated  in  one 
element,  and  hence  the  overall  force-deflection  behavior of  the  structure  can  be  mesh-
size-dependent if the softening is characterized by strain.  To avoid this, a characteristic 
length  (LCHAR)  may  be  defined.    This  is  the  length  of  specimen  (or  element)  that 
would  exhibit  the  defined  monotonic  stress-strain  relationship.    LS-DYNA  adjusts  the
stress-strain  relationship  after  ultimate  load  for  each  element,  such  that  all  elements 
irrespective  of  their  length  will  show  the  same  deflection  during  strain  softening  (i.e.  
between ultimate load and residual load).  Therefore, although deformation will still be 
concentrated  in  one  element,  the  load-deflection  behavior  should  be  the  same 
irrespective of element size.  For tensile behavior, ESOFT is similarly scaled. 
MAT_RC_BEAM - concrete 
17
18
16
15,19
20 
7 
7,9 
5,12 
8 
10 
11 
1 
4 
13
3,14
Figure M174-1 
Cyclic behavior is broadly suggested by Blakeley and Park [1973] as described in Park & 
Paulay  [1975];  the  stress-strain  response  lies  within  the  Park-Kent  envelope,  and  is 
characterized by stiff initial unloading response at slope EUNL followed by a less stiff 
response  if  it  unloads  to  less  than  half  the  current  strength.    Reloading  stiffness 
degrades with increasing strain. 
In  tension,  the  stress  rises  linearly  with  strain  until  a  tensile  limit  FT  is  reached.  
Thereafter the stiffness and strength decays with increasing strain at a rate ESOFT.  The 
stiffness  also  decays  such  that  unloading  always  returns  to  strain  at  which  the  stress 
most recently changed to tensile.
σult 
σy 
εsh 
εult 
Figure M174-2 
MAT_RC_BEAM – reinforcement – 
RREINF = 4.0 
6,8
3,5
9,11
12,14  15 
13 
7 
1 
10 
Figure M174-3 
Monotonic loading of the reinforcement results in the stress-strain curve shown, which 
is parabolic between εsh and εult.  The same curve acts as an envelope on the hysteretic 
behavior, when the x-axis is cumulative plastic strain.  
Unloading from the yielded condition is elastic until the load reverses.  Thereafter, the 
Bauschinger  Effect  (reduction  in  stiffness  at  stresses  less  than  yield  during  cyclic 
deformation)  is  represented  by  following  a  Ramberg-Osgood  relationship  until  the 
yield stress is reached: 
𝜀 − 𝜀𝑠 = (
) {1 + (
𝜎𝐶𝐻
𝑟−1
)
}
where 𝜀 and 𝜎 are strain and stress, 𝜀𝑠
and r and 𝜎𝐶𝐻
 are as defined below 
 is the strain at zero stress, E is Young’s Modulus, 
Two  options  are  given  for  calculation  r  and  𝜎𝐶𝐻,  which  is  performed  at  each  stress 
reversal: 
1. 
2. 
If RREINF is input as -1, r and σCH are calculated internally from formulae given 
in  Kent  and  Park.    Parameter  r  depends  on  the  number  of  stress  reversals.  
Parameter 𝜎𝐶𝐻  depends  on  the  plastic  strain  that  occurred  between  the  previ-
ous  two  stress  reversals.    The  formulae  were  statistically  derived  from  experi-
ments,  but  may  not  fit  all  circumstances.    In  particular,  large  differences  in 
behavior  may  be  caused  by  the  presence  or  absence  of  small  stress  reversals 
such  as  could  be  caused  by  high  frequency  oscillations.    Therefore,  results 
might sometimes be unduly sensitive to small changes in the input data. 
If  RREINF  is  entered  by  the  user  or  left  blank,  r  is  held  constant  while  𝜎𝐶𝐻  is 
calculated  on  each  reversal  such  that  the  Ramberg-Osgood  curve  meets  the 
monotonic  stress-strain  curve  at  the  point  from  which  it  last  unloaded,  e.g.  
points  6  and  8  are  coincident  in  the  graph  below.    The  default  setting 
RREINF = 4.0  gives  similar  hysteresis  behavior  to  that  described  by  Kent  & 
Park but is unlikely to be so sensitive to small changes of input data. 
Output: 
It is recommended to use BEAMIP on *DATABASE_EXTENT_BINARY to request stress 
and  strain  output  at  the  individual  integration  points.    If  this  is  done,  for  MAT_RC_-
BEAM only, element curvature is written to the output files in place of plastic strain.  In 
the  post-processor,  select  “plastic  strain”  to  display  curvature  (whichever  of  the 
curvatures  about  local  y  and  z  axes  has  greatest  absolute  value  will  be  plotted).  
Alternatively,  select  “axial  strain”  to  display  the  total  axial  strain  (elastic  +  plastic)  at 
that  integration  point;  this  can  be  combined  with  axial  stress  to  create  hysteresis  plots 
such as those shown above.
*MAT_VISCOELASTIC_THERMAL 
This is Material Type 175.  This material model provides a general viscoelastic Maxwell 
model having up to 12 terms in the prony series expansion and is useful for modeling 
dense  continuum  rubbers  and  solid  explosives.    Either  the  coefficients  of  the  prony 
series  expansion  or  a  relaxation  curve  may  be  specified  to  define  the  viscoelastic 
deviatoric and bulk behavior.  Note that   *MAT_GENERAL_VISCOELASTIC (Material 
Type 76) has all the capability of *MAT_VISCOELASTIC_THERMAL, and additionally 
offers more terms (18) in the prony series expansion and an optional scaling of material 
properties with moisture content. 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
4 
BULK 
PCF 
Type 
A8 
F 
F 
F 
5 
EF 
F 
6 
TREF 
F 
7 
A 
F 
8 
B 
F 
If fitting is done from a relaxation curve, specify fitting parameters on card 2, otherwise
if constants are set on Viscoelastic Constant Cards LEAVE THIS CARD BLANK. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
NT 
BSTART 
TRAMP 
LCIDK 
NTK 
BSTARTK  TRAMPK 
Type 
F 
I 
F 
F 
F 
I 
F 
F 
Viscoelastic Constant Cards.  Up to 6 cards may be input.  A keyword card (with a 
“*” in column 1) terminates this input if less than 6 cards are used.  These cards are not 
needed if relaxation data is defined.  The number of terms for the shear behavior may 
differ from that for the bulk behavior: simply insert zero if a term is not included.  If an 
elastic layer is defined you only need to define GI and KI (note in an elastic layer only 
one card is needed). 
 Optional 
Variable 
Type 
1 
Gi 
F 
2 
BETAi 
F 
3 
Ki 
F 
4 
5 
6 
7 
8 
BETAKi
VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density. 
BULK 
Elastic bulk modulus. 
PCF 
Tensile pressure elimination flag for solid elements only.  If set to
unity tensile pressures are set to zero. 
EF 
Elastic flag: 
EQ.0:  the later is viscoelastic 
EQ.1:  the layer is elastic 
TREF 
A 
B 
LCID 
NT 
Reference  temperature  for  shift  function  (must  be  greater  than
zero). 
Coefficient for the Arrhenius and the Williams-Landel-Ferry shift 
functions. 
Coefficient for the Williams-Landel-Ferry shift function. 
Load curve ID for deviatoric behavior if constants, 𝐺𝑖, and 𝛽𝑖 are 
determined via a least squares fit.  This relaxation curve is shown
below. 
Number of terms in shear fit.  If zero the default is 6.  Fewer than
NT  terms  will  be  used  if  the  fit  produces  one  or  more  negative
shear moduli.  Currently, the maximum number is set to 6. 
BSTART 
In the fit, 𝛽1  is set to zero, 𝛽2  is set to BSTART, 𝛽3  is 10 times 𝛽2, 
𝛽4 is 10 times 𝛽3 , and so on.  If zero, BSTART is determined by an
iterative trial and error scheme. 
TRAMP 
Optional ramp time for loading. 
LCIDK 
Load  curve  ID  for  bulk  behavior  if  constants,  𝐾𝑖,  and  𝛽𝜅𝑖    are 
determined via a least squares fit.  This relaxation curve is shown
below. 
NTK 
Number  of  terms  desired  in  bulk  fit.    If  zero  the  default  is  6.
Currently, the maximum number is set to 6.
BSTARTK 
*MAT_VISCOELASTIC_THERMAL 
DESCRIPTION
In the fit, 𝛽𝜅1  is set to zero, 𝛽𝜅2  is set to BSTARTK, 𝛽𝜅3 is 10 times 
𝛽𝜅2,  𝛽𝜅4  is  10  times  𝛽𝜅3  ,  and  so  on.    If  zero,  BSTARTK  is 
determined by an iterative trial and error scheme. 
TRAMPK 
Optional ramp time for bulk loading. 
Gi 
Optional shear relaxation modulus for the ith term 
BETAi 
Optional shear decay constant for the ith term 
Ki 
Optional bulk relaxation modulus for the ith term 
BETAKi 
Optional bulk decay constant for the ith term
σ∕ε
TRAMP
10n
10n+1 10n+2 10n+3
time
optional ramp time for loading
Figure M175-1.  Relaxation curve.  This curve defines stress versus time where
time  is  defined  on  a  logarithmic  scale.    For best  results,  the  points  defined  in
the load curve should be equally spaced on the logarithmic scale.  Furthermore,
Furthermore,  the  load  curve  should  be  smooth  and  defined  in  the  positive
quadrant.  If nonphysical values are determined by least squares fit, LS-DYNA
will terminate with an error message after the initialization phase is completed.
If  the  ramp  time  for  loading  is  included,  then  the  relaxation  which  occurs
during the loading phase is taken into account.  This effect may or may not be
important 
Remarks: 
Rate  effects  are  taken  into  accounted  through  linear  viscoelasticity  by  a  convolution 
integral of the form: 
𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)
∂𝜀𝑘𝑙
∂𝜏
𝑑𝜏
where 𝑔𝑖𝑗𝑘𝑙(𝑡−𝜏) is the relaxation functions for the different stress measures.  This stress is 
added to the stress tensor determined from the strain energy functional.     
If we wish to include only simple rate effects, the relaxation function is represented by 
six terms from the Prony series: 
𝑔(𝑡) = ∑ 𝐺𝑚𝑒−𝛽𝑚𝑡
𝑚=1
We  characterize  this  in  the  input  by  shear  moduli,  𝐺𝑖,  and  decay  constants,  𝛽𝑖.    An 
arbitrary number of terms, up to 6, may be used when applying the viscoelastic model. 
For volumetric relaxation, the relaxation function is also represented by the Prony series 
in terms of bulk moduli: 
𝑘(𝑡) = ∑ 𝐾𝑚𝑒−𝛽𝑘𝑚𝑡
𝑚=1
The Arrhenius and Williams-Landel-Ferry (WLF) shift functions account for the effects 
of the temperature on the stress relaxation.  A scaled time, t’, 
𝑡′ = ∫ Φ(𝑇)𝑑𝑡
is  used  in  the  relaxation  function  instead  of  the  physical  time.    The  Arrhenius  shift 
function is 
Φ(𝑇) = exp [−𝐴 (
−
𝑇REF
)] 
and the Williams-Landel-Ferry shift function is 
Φ(𝑇) = exp (−𝐴
𝑇 − 𝑇REF
𝐵 + 𝑇 − 𝑇REF
) 
If  all  three  values  (TREF,  A,  and  B)  are  not  zero,  the  WLF  function  is  used;  the 
Arrhenius function is used if B is zero; and no scaling is applied if all three values are 
zero. 
.
*MAT_QUASILINEAR_VISCOELASTIC 
Purpose:    This  is  Material  Type  176.    This  is  a  quasi-linear,  isotropic,  viscoelastic 
material based on a one-dimensional model by Fung [1993], which represents biological 
soft tissues such as brain, skin, kidney, spleen, etc.  This model is implemented for solid 
and shell elements.  The formulation has recently been changed to allow larger strains, 
and,  in  general,  will  not  give  the  same  results  as  the  previous  implementation  which 
remains the default. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
K 
F 
Default 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
5 
LC1 
LC2 
I 
0 
4 
I 
0 
5 
Variable 
SO 
E_MIN 
E_MAX 
GAMA1 
GAMA2 
Type 
F 
F 
F 
F 
F 
6 
N 
F 
6 
6 
K 
F 
7 
GSTART 
F 
1/TMAX 
7 
EH 
F 
Default 
0.0 
-0.9 
5.1 
0.0 
0.0 
0.0 
0.0 
Viscoelastic Constant Card 1.  Additional Card for LC1 = 0. 
  Card 3 
Variable 
1 
G1 
2 
BETA1 
Type 
F 
F 
3 
G2 
F 
4 
BETA2 
F 
5 
G3 
F 
6 
BETA3 
F 
7 
G4 
F 
8 
M 
F 
6 
8 
FORM 
I 
0 
8 
BETA4
Viscoelastic Constant Card 2.  Additional Card for LC1 = 0. 
  Card 4 
Variable 
1 
G5 
2 
BETA5 
Type 
F 
F 
3 
G6 
F 
4 
BETA6 
F 
5 
G7 
F 
6 
BETA7 
F 
7 
G8 
F 
8 
BETA8 
F 
Viscoelastic Constant Card 3.  Additional Card for LC1 = 0. 
  Card 5 
Variable 
1 
G9 
2 
3 
4 
5 
6 
7 
8 
BETA9 
G10 
BETA10 
G11 
BETA11 
G12 
BETA12 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Instantaneous Elastic Reponses Card.  Additional Card for LC2 = 0. 
Card 
Variable 
1 
C1 
Type 
F 
2 
C2 
F 
3 
C3 
F 
4 
C4 
F 
5 
C5 
F 
6 
C6 
F 
7 
8 
  VARIABLE   
DESCRIPTION
MID 
RO 
K 
LC1 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Bulk modulus. 
Load curve ID that defines the relaxation function in shear.  This
curve is used to fit the coefficients Gi and BETAi.  If zero, define 
the coefficients directly.  The latter is recommended.
VARIABLE   
LC2 
N 
DESCRIPTION
Load  curve  ID  that  defines  the  instantaneous  elastic  response  in 
compression and tension.  If zero, define the coefficients directly.
Symmetry  is  not  assumed  if  only  the  tension  side  is  define;  therefore,
defining the response in tension only, may lead to nonphysical behavior
in  compression.    Also,  this  curve  should  give  a  softening  response  for 
increasing  strain  without  any  negative  or  zero  slopes.    A  stiffening
curve or one with negative slopes is generally unstable. 
Number of terms used in the Prony series, a number less than or
equal  to  6.    This  number  should  be  equal  to  the  number  of
decades  of  time  covered  by  the  experimental  data.    Define  this
number if LC1 is nonzero.  Carefully check the fit in the d3hsp file 
to  ensure  that  it  is  valid,  since  the  least  square  fit  is  not  always
reliable. 
GSTART 
Starting  value  for  least  square  fit.    If  zero,  a  default  value  is  set
equal to the inverse of the largest time in the experiment.  Define
this number if LC1 is nonzero. 
M 
SO 
Number  of  terms  used  to  determine  the  instantaneous  elastic
response.  This variable is ignored with the new formulation but
is kept for compatibility with the previous input. 
Strain  (logarithmic)  output  option  to  control  what  is  written  as
component 7 to the d3plot database.  (LS-PrePost always blindly 
labels  this  component  as  effective  plastic  strain.)    The  maximum
values are updated for each element each time step: 
EQ.0.0: maximum  principal  strain  that  occurs  during  the
calculation, 
EQ.1.0: maximum magnitude of the principal strain values that 
occurs during the calculation, 
EQ.2.0: maximum  effective  strain  that  occurs  during  the
calculation. 
E_MIN 
Minimum  strain  used  to  generate  the  load  curve  from  𝐶𝑖.    The 
default range is -0.9 to 5.1.  The  computed solution will be more 
accurate  if  the  user  specifies  the  range  used  to  fit  the  𝐶𝑖.    Linear 
extrapolation is used outside the specified range. 
E_MAX 
Maximum strain used to generate the load curve from 𝐶𝑖.
*MAT_QUASILINEAR_VISCOELASTIC 
DESCRIPTION
K 
Material  failure  parameter  that  controls  the  volume  enclosed  by 
the failure surface, see *MAT_SIMPLIFIED_RUBBER. 
LE.0.0:  ignore failure criterion; 
GT.0.0: use actual K value for failure criterions. 
GAMA1 
Material failure parameter, see *MAT_SIMPLIFIED_RUBBER and 
Figure M181-1. 
GAMA2 
Material failure parameter, see *MAT_SIMPLIFIED_RUBBER. 
EH 
Damage parameter, see *MAT_SIMPLIFIED_RUBBER. 
FORM 
Gi 
BETAi 
Formulation  of  model.    FORM =  0  gives  the  original  model 
developed by Fung, which always relaxes to a zero stress state as
time  approaches  infinity,  and  FORM =  1  gives  the  alternative 
model,  which  relaxes  to  the  quasi-static  elastic  response.    In 
general,  the  two  formulations  won’t  give  the  same  responses.
Formulation, FORM = -1, is an improvement on FORM = 0 where 
the instantaneous elastic response is used in the viscoelastic stress
update, not just in the relaxation, as in FORM = 0.  Consequently, 
the constants for the elastic response do not need to be scaled. 
Coefficients of the relaxation function.  The number of coefficients
is  currently  limited  to  6  although  12  may  be  read  in  to  maintain
compatibility with the previous formulation’s input.  Define these
coefficients  if  LC1  is  set  to  zero.    At  least  2  coefficients  must  be 
nonzero. 
Decay  constants  of  the  relaxation  function. 
  Define  these
coefficients  if  LC1  is  set  to  zero.    The  number  of  coefficients  is
currently  limited  to  6  although  12  may  be  read  in  to  maintain
compatibility with the previous formulation’s input. 
Ci 
Coefficients of the instantaneous elastic response in  compression
and tension.   Define these coefficients only if LC2 is set to zero. 
Remarks: 
The equations for the original model (FORM = 0) are given as: 
𝜎𝑉(𝑡) = ∫ 𝐺(𝑡 − 𝜏)
∂𝜎𝜀[𝜀(𝜏)]
∂𝜀
∂𝜀
∂𝜏
𝑑𝜏
𝐺(𝑡) = ∑ 𝐺𝑖
𝑒−𝛽𝑡 
𝑖=1
𝜎𝜀(𝜀) = ∑ 𝐶𝑖
𝜀𝑖 
𝑖=1
where  G  is  the  shear  modulus.    Effective  strain  (which  can  be  written  to  the  d3plot 
database) is calculated as follows: 
𝜀effective = √
𝜀𝑖𝑗𝜀𝑖𝑗 
The  polynomial  for  instantaneous  elastic  response  should  contain  only  odd  terms  if 
symmetric tension-compression response is desired. 
The  new  model  (FORM = 1)  is  based  on  the  hyperelastic  model  used  *MAT_SIMPLI-
FIED_RUBBER  assuming  incompressibility.    The  one-dimensional  expression  for 
𝜎𝜀generates  the  uniaxial  stress-strain  curve  and  an  additional  visco-elastic  term  is 
added on, 
𝜎(𝜀, 𝑡) = 𝜎𝑆𝑅(𝜀) + 𝜎𝑉(𝑡) 
𝜎𝑉(𝑡) = ∫ 𝐺(𝑡 − 𝜏)
∂𝜀
∂𝜏
𝑑𝜏
where  the  first  term  to  the  right  of  the  equals  sign  is  the  hyperelastic  stress  and  the 
second  is  the  viscoelastic  stress.    Unlike  the  previous  formulation,  where  the  stress 
always relaxed to zero, the current formulation relaxes to the hyperelastic stress.
*MAT_HILL_FOAM 
Purpose:    This  is  Material  Type  177.    This  is  a  highly  compressible  foam  based  on  the 
strain-energy function proposed by Hill [1979]; also see Storakers [1986].  Poisson’s ratio 
effects are taken into account. 
5 
6 
7 
8 
MU 
LCID 
FITTYPE 
LCSR 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
K 
F 
Default 
none 
none 
none 
4 
N 
F 
0 
F 
0 
Material Constant Card 1.  Additional card for LCID = 0. 
  Card 2 
Variable 
1 
C1 
Type 
F 
2 
C2 
F 
3 
C3 
F 
4 
C4 
F 
5 
C5 
F 
Material Constant Card 2.  Additional card for LCID = 0. 
3 
B3 
F 
3 
4 
B4 
F 
4 
5 
B5 
F 
5 
  Card 3 
Variable 
1 
B1 
Type 
F 
  Card 4 
Variable 
Type 
1 
R 
F 
2 
B2 
F 
2 
M 
F 
I 
0 
6 
C6 
F 
6 
B6 
F 
6 
I 
0 
7 
C7 
F 
7 
B7 
F 
7 
I 
0 
8 
C8 
F 
8 
B8 
F
VARIABLE   
DESCRIPTION
MID 
RO 
K 
N 
MU 
LCID 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Bulk modulus.  This modulus is used for determining the contact
interface stiffness. 
Material  constant.    Define  if  LCID = 0  below;  otherwise,  N  is  fit 
from the load curve data.  See equations below. 
Damping coefficient. 
Load  curve  ID  that  defines  the  force  per  unit  area  versus  the
stretch ratio.  This curve can be given for either uniaxial or biaxial
data depending on FITTYPE. 
FITTYPE 
Type of fit: 
EQ.1: uniaxial data, 
EQ.2: biaxial data, 
EQ.3: pure shear data. 
LCSR 
Load curve ID that defines the uniaxial or biaxial stretch ratio  versus the transverse stretch ratio. 
Material  constants.    See  equations  below.    Define  up  to  8
coefficients if LCID = 0. 
Material  constants.    See  equations  below.    Define  up  to  8
coefficients if LCID = 0. 
Mullins effect model r coefficient 
Mullins effect model m coefficient 
Ci 
Bi 
R 
M 
Remarks: 
If load curve data is defined, the fit generated by LS-DYNA must be closely checked in 
the D3HSP output file.  It may occur that the nonlinear least squares procedure in LS-
DYNA, which is used to fit the data, is inadequate. 
The Hill strain energy density function for this highly compressible foam is given by:
𝑊 = ∑
𝑗=1
𝐶𝑗
𝑏𝑗
𝑏𝑗 + 𝜆2
𝑏𝑗 + 𝜆3
[𝜆1
𝑏𝑗 − 3 +
(𝐽−𝑛𝑏𝑗 − 1)] 
where  𝐶𝑗,  𝑏𝑗,  and  n  are  material  constants  and  𝐽 = 𝜆1𝜆2𝜆3  represents  the  ratio  of  the 
deformed  to  the  undeformed  state.    The  constant  m  is  internally  set  to  4.    In  case 
number  of  points  in  the  curve  is  less  than  8,  then  m  is  set  to  the  number  of  points 
divided by 2.  The principal Cauchy stresses are 
𝑡𝑖 = ∑
𝑗=1
𝐶𝑗
𝑏𝑗 − 𝐽−𝑛𝑏𝑗]    𝑖 = 1,2,3 
[𝜆𝑖
From the above equations the shear modulus is:
and the bulk modulus is: 
𝜇 =
∑ 𝐶𝑗𝑏𝑗
𝑗=1
𝐾 = 2𝜇 (𝑛 +
) 
The value for K defined in the input is used in the calculation of contact forces and for 
the  material  time  step.    Generally,  this  value  should  be  equal  to  or  greater  that  the  K 
given in the above equation.
*MAT_VISCOELASTIC_HILL_FOAM 
Purpose:    This  is  Material  Type  178.    This  is  a  highly  compressible  foam  based  on  the 
strain-energy function proposed by Hill [1979]; also see Storakers [1986].  The extension 
to include large strain viscoelasticity is due to Feng and Hallquist [2002]. 
5 
6 
7 
8 
MU 
LCID 
FITTYPE 
LCSR 
4 
N 
F 
0 
4 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
K 
F 
Default 
none 
none 
none 
  Card 2 
1 
2 
3 
Variable 
LCVE 
NT 
GSTART 
Type 
Default 
I 
0 
F 
6 
F 
1/TMAX
F 
0.05 
5 
Material Constant Card 1.  Additional card for LCID = 0. 
  Card 3 
Variable 
1 
C1 
Type 
F 
2 
C2 
F 
3 
C3 
F 
4 
C4 
F 
5 
C5 
F 
Material Constant Card 2.  Additional card for LCID = 0. 
  Card 4 
Variable 
1 
B1 
Type 
F 
2 
B2 
F 
3 
B3 
F 
4 
B4 
F 
5 
B5 
F 
I 
0 
6 
6 
C6 
F 
6 
B6 
F 
I 
0 
7 
7 
C7 
F 
7 
B7 
F 
I 
0 
8 
8 
C8 
F 
8 
B8
Viscoelastic Constant Cards.  Up to 12 cards may be input.  A keyword card (with a 
“*” in column 1) terminates this input if less than 12 cards are used.  
  Card 5 
Variable 
Type 
1 
GI 
F 
2 
3 
4 
5 
6 
7 
8 
BETAI 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
K 
N 
MU 
LCID 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Bulk modulus.  This modulus is used for determining the contact
interface stiffness. 
Material  constant.    Define  if  LCID = 0  below;  otherwise,  N  is  fit 
from the load curve data.  See equations below. 
Damping coefficient (0.05 < recommended value < 0.50; default is 
0.05). 
Load  curve  ID  that  defines  the  force  per  unit  area  versus  the 
stretch ratio.  This curve can be given for either uniaxial or biaxial
data depending on FITTYPE.  Load curve LCSR below must also
be defined. 
FITTYPE 
Type of fit: 
EQ.1: uniaxial data, 
EQ.2: biaxial data. 
LCSR 
LCVE 
Load curve ID that defines the uniaxial or biaxial stress ratio  versus the transverse stretch ratio. 
Optional  load  curve  ID  that  defines  the  relaxation  function  in
shear.  This  curve is used to fit the coefficients Gi and BETAi.  If 
zero, define the coefficients directly.  The latter is recommended.
VARIABLE   
NT 
DESCRIPTION
Number of terms used to fit the Prony series, which is a number
less  than  or  equal  to  12.    This  number  should  be  equal  to  the
number  of  decades  of  time  covered  by  the  experimental  data. 
Define this number if LCVE is nonzero.  Carefully check the fit in
the D3HSP file to ensure that it is valid, since the least square fit is
not always reliable. 
GSTART 
Starting  value  for  least  square  fit.    If  zero,  a  default  value  is  set
equal to the inverse of the largest time in the experiment.   Define
this  number  if  LC1  is  nonzero,  Ci,  Material  constants.    See 
equations below.  Define up to 8 coefficients. 
Ci 
Bi 
GI 
Material  constants.    See  equations  below.    Define  up  to  8
coefficients if LCID = 0. 
Material  constants.    See  equations  below.    Define  up  to  8
coefficients if LCID = 0. 
Optional shear relaxation modulus for the ith term 
BETAI 
Optional decay constant if ith term 
Remarks: 
If load curve data is defined, the fit generated by LS-DYNA must be closely checked in 
the D3HSP output file.  It may occur that the nonlinear least squares procedure in LS-
DYNA, which is used to fit the data, is inadequate. 
The Hill strain energy density function for this highly compressible foam is given by: 
𝑝𝑛+1 = 𝑝𝑛𝑒−𝛽⋅𝛥𝑡 + 𝐾𝜀̇𝑘𝑘 (
1 − 𝑒−𝛽⋅𝛥𝑡
)         where  𝛽 = |𝐵𝐸𝑇𝐴| 
where  𝐶𝑗,  𝑏𝑗,  and  n  are  material  constants  and  𝐽 = 𝜆1𝜆2𝜆3  represents  the  ratio  of  the 
deformed to the undeformed state.  The principal Cauchy stresses are 
𝑡𝑖 = ∑
𝑗=1
𝐶𝑗
𝑏𝑗 − 𝐽−𝑛𝑏𝑗]    𝑖 = 1,2,3 
[𝜆𝑖
From the above equations the shear modulus is: 
𝜇 =
∑ 𝐶𝑗𝑏𝑗
𝑗=1
and the bulk modulus is:
𝐾 = 2𝜇 (𝑛 +
) 
The value for K defined in the input is used in the calculation of contact forces and for 
the  material  time  step.    Generally,  this  value  should  be  equal  to  or  greater  that  the  K 
given in the above equation. 
Rate  effects  are  taken  into  account  through  linear  viscoelasticity  by  a  convolution 
integral of the form: 
𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙
(𝑡 − 𝜏)
∂𝜀𝑘𝑙
∂𝜏
𝑑𝜏 
or in terms of the second Piola-Kirchhoff stress, 𝑆𝑖𝑗, and Green's strain tensor, 𝐸𝑖𝑗, 
𝑆𝑖𝑗 = ∫ 𝐺𝑖𝑗𝑘𝑙
(𝑡 − 𝜏)
∂ 𝐸𝑘𝑙
∂𝜏
𝑑𝜏 
where  𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)  and  𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏)    are  the  relaxation  functions  for  the  different  stress 
measures.    This  stress  is  added  to  the  stress  tensor  determined  from  the  strain  energy 
functional. 
If we wish to include only simple rate effects, the relaxation function is represented by 
six terms from the Prony series: 
given by, 
𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚
𝑚=1
𝑒−𝛽 𝑡 
𝑔(𝑡) = ∑ 𝐺𝑖𝑒−𝛽𝑖 𝑡
𝑖=1
This  model  is  effectively  a  Maxwell  fluid  which  consists  of  a  dampers  and  springs  in 
series.  We  characterize this in the input by  shear moduli, 𝐺𝑖, and  decay constants,  𝛽𝑖.  
The viscoelastic behavior is optional and an arbitrary number of terms may be used.
*MAT_LOW_DENSITY_SYNTHETIC_FOAM_{OPTION} 
This is Material Type 179 (and 180 if the ORTHO option below is active) for modeling 
rate independent low density foams, which have the property that the hysteresis in the 
loading-unloading  curve  is  considerably  reduced  after  the  first  loading  cycle.    In  this 
material we assume that the loading-unloading curve is identical after the first cycle of 
loading  is  completed  and  that  the  damage  is  isotropic,  i.e.,  the  behavior  after  the  first 
cycle  of  loading  in the  orthogonal  directions  also  follows  the  second  curve.    The  main 
application at this time is to model the observed behavior in the compressible synthetic 
foams  that  are  used  in  some  bumper  designs.    Tables  may  be  used  in  place  of  load 
curves to account for strain rate effects. 
Available options include: 
<BLANK> 
ORTHO 
WITH_FAILURE 
ORTHO_WITH_FAILURE 
If  the  foam  develops  orthotropic  behavior,  i.e.,  after  the  first  loading  and  unloading 
cycle  the  material  in  the  orthogonal  directions  are  unaffected  then  the  ORTHO  option 
should  be  used.    If  the  ORTHO  option  is  active  the  directionality  of  the  loading  is 
stored.  This option is requires additional storage to store the history variables related to 
the orthogonality and is slightly more expensive. 
An optional failure criterion is included.  A description of the failure model is provided 
below for material type 181, *MAT_SIMPLIFIED_RUBBER/FOAM. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
5 
LCID1 
LCID2 
F 
F 
Default 
6 
HU 
F 
1. 
7 
8 
BETA 
DAMP 
F 
F 
0.05
Card 2 
1 
2 
3 
4 
5 
6 
7 
Variable 
SHAPE 
FAIL 
BVFLAG 
ED 
BETA1 
KCON 
REF 
Type 
F 
F 
F 
F 
F 
F 
F 
8 
TC 
F 
Default 
1.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
1.E+20 
Additional card for LCID1 < 0.  
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RFLAG 
DTRT 
Type 
F 
F 
Default 
0.0 
0.0 
Additional card for WITH_FAILURE keyword option.  
  Card 4 
Variable 
Type 
1 
K 
F 
2 
3 
GAMA1 
GAMA2 
F 
F 
4 
EH 
F 
5 
6 
7 
8 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s  modulus.    This  modulus  is  used  if  the  elongations  are
tensile as described for the *MAT_LOW_DENSITY_FOAM.
VARIABLE   
DESCRIPTION
LCID1 
Load curve or table ID: 
LCID2 
HU 
BETA 
DAMP 
GT.0: Load curve ID, see *DEFINE_CURVE, for nominal stress 
versus strain for the undamaged material. 
LT.0:  -LCID1  is  Table  ID,  see  *DEFINE_TABLE,  for  nominal 
stress  versus  strain  for  the  undamaged  material  as  a
function of strain rate 
Load curve or table ID.  The load curve ID, see *DEFINE_CURVE, 
defines the nominal stress versus strain for the damaged material.
The  table  ID,  see  *DEFINE_TABLE,  defines  the  nominal  stress 
versus strain for the damaged material as a function of strain rate
Hysteretic  unloading  factor  between  0  and  1  (default = 1,  i.e.,  no 
energy dissipation), see also Figure M179-1. 
β, decay constant to model creep in unloading 
Viscous  coefficient  (.05 < recommended  value  <.50)  to  model 
damping effects. 
LT.0.0: |DAMP|  is  the  load  curve  ID,  which  defines  the
damping constant as a function of the maximum strain
in compression defined as: 
𝜀max = max(1 − 𝜆1, 1 − 𝜆2, 1. −𝜆3). 
In  tension,  the  damping  constant  is  set  to  the  value  corre-
sponding  to  the  strain  at  0.    The  abscissa  should  be  defined 
from 0 to 1. 
SHAPE 
Shape  factor  for  unloading.    Active  for  nonzero  values  of  the
hysteretic  unloading  factor.    Values  less  than  one  reduces  the
energy dissipation and greater than one increases dissipation, see
also Figure M179-1 
FAIL 
Failure option after cutoff stress is reached: 
EQ.0.0: tensile stress remains at cut-off value, 
EQ.1.0: tensile stress is reset to zero. 
BVFLAG 
Bulk viscosity activation flag, see remark below: 
EQ.0.0: no bulk viscosity (recommended), 
EQ.1.0: bulk viscosity active.
ED 
BETA1 
KCON 
*MAT_LOW_DENSITY_SYNTHETIC_FOAM 
DESCRIPTION
Optional  Young's  relaxation  modulus,  𝐸𝑑,  for  rate  effects.    See 
comments below. 
Optional decay constant, 𝛽1. 
Stiffness  coefficient  for  contact  interface  stiffness.    If  undefined
the maximum slope in stress vs.  strain curve is used.  When the
maximum slope is taken for the contact, the time step size for this
material  is  reduced  for  stability.    In  some  cases  Δt  may  be 
significantly  smaller,  and  defining  a  reasonable  stiffness  is
recommended. 
REF 
Use  reference  geometry  to  initialize  the  stress  tensor.    The
reference geometry is defined by the keyword:*INITIAL_FOAM_-
REFERENCE_GEOMETRY . 
EQ.0.0: off, 
EQ.1.0: on. 
TC 
Tension cut-off stress 
RFLAG 
Rate type for input: 
EQ.0.0: LCID1 and LCID2 should be input as functions of true
strain rate 
EQ.1.0: LCID1  and  LCID2  should  be  input  as  functions  of
engineering strain rate. 
DTRT 
Strain rate averaging flag: 
EQ.0.0: use weighted running average 
LT.0.0:  average the last 11 values 
GT.0.0:  average over the last DTRT time units. 
K 
Material  failure  parameter  that  controls  the  volume  enclosed  by
the failure surface. 
LE.0.0:  ignore failure criterion; 
GT.0.0: use actual K value for failure criterions. 
GAMA1 
Material  failure  parameter,  see  equations  below  and  Figure 
M181-1. 
GAMA2 
Material failure parameter, see equations below.
Loading curve
for first cycle
Loading curve for second
and subsequent cycles
Strain
Figure M179-1.  Loading and reloading curves. 
  VARIABLE   
DESCRIPTION
EH 
Damage parameter. 
Remarks: 
This  model  is  based  on  *MAT_LOW_DENSITY_FOAM.    The  uniaxial  response  is 
shown below with a large shape factor and small hysteretic factor.  If the shape factor is 
not used, the unloading will occur on the loading curve for the second and subsequent 
cycles. 
The damage is defined as the ratio of the current volume strain to the maximum volume 
strain, and it is used to interpolate between the responses defined by LCID1 and LCID2.  
HU defines a hysteretic scale factor that is applied to the stress interpolated from LCID1 
and LCID2,  
𝜎 = [HU + (1 − HU) × min (1,
𝑒int
max)
𝑒int
] 𝜎(LCID1,LCID2) 
where eint is the internal energy and S is the shape factor.  Setting HU to 1 results in a 
scale  factor  of  1.    Setting  HU  close  to  zero  scales  the  stress  by  the  ratio  of  the  internal
energy  to  the  maximum  internal  energy  raised  to  the  power  S,  resulting  in  the  stress 
being reduced when the strain is low.
*MAT_SIMPLIFIED_RUBBER/FOAM_{OPTION} 
This  is  Material  Type  181.    This  material  model  provides  a  rubber  and  foam  model 
defined  by  a  single  uniaxial  load  curve  or  by  a  family  of  uniaxial  curves  at  discrete 
strain rates.  The definition of hysteretic unloading is optional and can be realized via a 
single  uniaxial  unloading  curve  or  a  two-parameter  formulation  (starting  with  971 
release  R5).    The  foam  formulation  is  triggered  by  defining  a  Poisson’s  ratio.    This 
material may be used with both shell and solid elements. 
Available options include: 
<BLANK> 
WITH_FAILURE 
LOG_LOG_INTERPOLATION 
When  the  WITH_FAILURE  keyword  option  is  active,  a  strain  based  failure  surface  is 
defined  suitable  for  incompressible  polymers  modeling  failure  in  both  tension  and 
compression. 
This  material 
collaboration with Paul Du Bois, LSTC, and Prof.  Dave J.  Benson, UCSD. 
law  has  been  developed  at  DaimlerChrysler,  Sindelfingen, 
in 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
KM 
F 
3 
4 
MU 
F 
4 
5 
G 
F 
5 
6 
7 
8 
SIGF 
REF 
PRTEN 
F 
6 
F 
7 
F 
8 
Variable 
SGL 
SW 
ST 
LC /TBID  TENSION 
RTYPE 
AVGOPT  PR/BETA 
Type 
F 
F 
F 
F 
F 
F 
F
Additional card required for WITH_FAILURE option.  Otherwise skip this card. 
5 
6 
7 
8 
  Card 3 
Variable 
Type 
1 
K 
F 
2 
3 
GAMA1 
GAMA2 
F 
F 
4 
EH 
F 
Optional Parameter Card. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCUNLD 
HU 
SHAPE 
STOL 
VISCO 
Type 
F 
F 
F 
F 
F 
Optional Viscoelastic Constants Cards.  Up to 12 card in format 5 may be input.  A 
keyword  card  (with  a  “*”  in  column  1)  terminates  this  input  if  less  than  12  cards  are 
used. 
1 
Gi 
F 
  Card 5 
Variable 
Type 
Default 
2 
3 
4 
5 
6 
7 
8 
BETAi 
VFLAG 
F 
I 
0 
  VARIABLE   
DESCRIPTION
MID 
RO 
KM 
MU 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Linear bulk modulus. 
Damping coefficient (0.05 < recommended value < 0.50; default is 
0.10).
VARIABLE   
DESCRIPTION
G 
SIGF 
REF 
PRTEN 
SGL 
SW 
ST 
LC/TBID 
Shear  modulus  for  frequency  independent  damping.    Frequency
independent  damping  is  based  on  a  spring  and  slider  in  series.
The critical stress for the slider mechanism is SIGF defined below.
For  the  best  results,  the  value  of  G  should  be  250-1000  times 
greater than SIGF. 
Limit stress for frequency independent, frictional, damping. 
Use  reference  geometry  to  initialize  the  stress  tensor.    The
reference geometry is defined by the keyword:*INITIAL_FOAM_-
REFERENCE_GEOMETRY . 
EQ.0.0: off, 
EQ.1.0: on. 
The tensile Poisson’s ratio for shells (optional).  If PRTEN is zero,
PR/BETA  will  serve  as  the  Poisson’s  ratio  for  both  tension  and
compression in shells.  If PRTEN is nonzero, PR/BETA will serve 
only as the compressive Poisson’s ratio for shells.   
Specimen gauge length 
Specimen width 
Specimen thickness 
Load  curve  or  table  ID,  see  *DEFINE_TABLE,  defining  the  force 
versus actual change in the gauge length.  If SGL, SW, and ST are
set to unity (1.0), then curve LC is also engineering stress versus
engineering  strain.    If  the  table  definition  is  used  a  family  of
curves  are  defined  for  discrete  strain  rates.    The  load  curves 
should  cover  the  complete  range  of  expected  loading,  i.e.,  the
smallest stretch ratio to the largest. 
TENSION 
Parameter  that  controls  how  the  rate  effects  are  treated.
Applicable to the table definition. 
EQ.-1.0:  rate  effects  are  considered  during  tension  and 
compression loading, but not during unloading, 
EQ.0.0:  rate  effects  are  considered  for  compressive  loading
only, 
EQ.1.0:  rate  effects  are  treated  identically  in  tension  and
compression.
*MAT_SIMPLIFIED_RUBBER/FOAM 
DESCRIPTION
RTYPE 
Strain rate type if a table is defined: 
EQ.0.0: true strain rate, 
EQ.1.0: engineering strain rate 
AVGOPT 
Averaging  option  determine  strain  rate  to  reduce  numerical
noise. 
LT.0.0:  |AVGOPT| is a time window/interval over which the
strain rates are averaged. 
EQ.0.0: simple average of twelve time steps, 
EQ.1.0: running average of last 12 averages. 
PR/BETA 
If the value is specified between 0 and 0.5 exclusive, i.e., 
0 < PR < 0.50 
the  number  defined  here  is  taken  as  Poisson’s  ratio.    If  zero,  an
incompressible  rubber  like  behavior  is  assumed  and  a  default
value  of  0.495  is  used  internally.    If  a  Poisson’s  ratio  of  0.0  is
desired,  input  a  small  value  for  PR  such  as  0.001.    When  fully
integrated solid elements are used and when a nonzero Poisson’s
ratio  is  specified,  a  foam  material  is  assumed  and  selective-
reduced integration is not used due to the compressibility.  This is
true  even  if  PR  approaches  0.500.    If  any  other  value  excluding 
zero  is  defined,  then  BETA  is  taken  as  the  absolute  value  of  the
given number and a nearly incompressible rubber like behavior is
assumed. 
  An  incrementally  updated  mean  viscous  stress
develops according to the equation: 
𝑝𝑛+1 = 𝑝𝑛𝑒−𝛽𝛥𝑡 + 𝐾𝑚𝜀̇𝑘𝑘 (
1 − 𝑒−𝛽𝛥𝑡
),  
where 𝛽 = |BETA| and 𝐾𝑚 = KM.  The BETA parameter does not 
apply to highly compressible foam materials. 
K 
Material  failure  parameter  that  controls  the  volume  enclosed  by
the failure surface. 
LE.0.0:  ignore failure criterion; 
GT.0.0: use actual K value for failure criterions. 
GAMA1 
Material failure parameter, see equations below and Figure 181.1.
GAMA2 
Material failure parameter, see equations below.
VARIABLE   
DESCRIPTION
EH 
Damage parameter. 
LCUNLD 
HU 
SHAPE 
Load  curve,  see  *DEFINE_CURVE,  defining  the  force  versus 
actual  length  during  unloading.    The  unload  curve  should  cover
exactly  the  same  range  as  LC  or  the  load  curves  of  TBID  and  its
end  points  should  have  identical  values,  i.e.,  the  combination  of
LC  and  LCUNLD  or  the  first  curve  of  TBID  and  LCUNLD
describes  a  complete  cycle  of  loading  and  unloading.    See  also
material *MAT_083. 
Hysteretic unloading factor between 0 and 1 (default = 1., i.e.  no 
energy  dissipation),  see  also  material  *MAT_083  and  Figure 
M57-1.  This option is ignored if LCUNLD is used. 
Shape  factor  for  unloading.    Active  for  nonzero  values  of  the
hysteretic unloading factor HU.  Values less than one reduces the
energy dissipation and greater than one increases dissipation, see
also material *MAT_083 and Figure M57-1. 
STOL 
Tolerance in stability check, see remarks. 
VISCO 
Viscoelasticity formulation. 
EQ.0.0: purely elastic; 
EQ.1.0: visco-elastic formulation. 
Gi 
Optional shear relaxation modulus for the ith term 
BETAi 
Optional decay constant if ith term 
VFLAG 
Flag for the viscoelasticity formulation.  This appears only on the
first  line  defining  Gi,  BETAi,  and  VFLAG.    If  VFLAG = 0,  the 
standard  viscoelasticity  formulation  is  used  (the  default),  and  if
the
viscoelasticity 
the 
VFLAG = 1, 
instantaneous elastic stress is used. 
formulation  using
1 = λ
K = 30
2 = 1
K = 20
K = 1
K = 10
Figure M181-1.  Failure surface for polymer for ۂ1 = 0 and ۂ2 = 0.02. 
Remarks: 
The  frequency  independent  damping  is  obtained  by  the  having  a  spring  and  slider  in 
series as shown in the following sketch: 
The general failure criterion for polymers is proposed by Feng and Hallquist as 
friction
𝑓 (𝐼1, 𝐼2, 𝐼3) = (𝐼1 − 3) + Γ1(𝐼1 − 3)2 + Γ2(𝐼2 − 3) = 𝐾 
where 𝐾 is a material parameter which controls the size enclosed by the failure surface, 
and 𝐼1, 𝐼2 and 𝐼3 are the three invariants of right Cauchy-Green deformation tensor (𝐂) 
2 
2 + 𝜆3
2 + 𝜆2
𝐼1 = C𝑖𝑖 = 𝜆1
𝐼2 =
(C𝑖𝑖C𝑗𝑗 − C𝑖𝑗C𝑖𝑗) = 𝜆1
2 𝜆2
2 + 𝜆1
2 𝜆3
2 + 𝜆2
2 
2 𝜆3
𝐼3 = det(𝐂) = 𝜆1
with 𝜆𝑖 are the stretch ratios in three principal directions. 
2 𝜆2
2 
2 𝜆3
To  avoid  sudden  failure  and  numerical  difficulty,  material  failure,  which  is  usually  a 
time point, is modeled as a process of damage growth.  In this case, the two threshold
values are chosen as (1 - h)K and K, where h (also called EH) is a small number chosen 
based  on  experimental  results  reflecting  the  range  between  damage  initiation  and 
material failure. 
The damage is defined as function of 𝑓 : 
𝐷 =
⎧
{{
⎨
{{
⎩
[ 1 + cos
𝜋(𝑓 − 𝐾)
]
ℎ𝐾
    if    𝑓 ≤ (1 − ℎ)𝐾
    if    (1 − ℎ)𝐾 < 𝑓 < 𝐾
    if    𝑓 ≥ 𝐾
This  definition  indicates  that  damage  is  first-order  continuous.    Under  this  definition, 
the tangent stiffness matrix will be continuous.  The reduced stress considering damage 
effect is 
𝑜 
𝜎𝑖𝑗 = (1 − 𝐷)𝜎𝑖𝑗
𝑜  is  the  undamaged  stress.    It  is  assumed  that  prior  to  final  failure,  material 
where  𝜎𝑖𝑗
damage is recoverable.  Once material failure occurs, damage will become permanent. 
The LOG_LOG_INTERPOLATION option interpolates the strain rate effect in the table 
TBID using log-log interpolation. 
Bad choices of curves for the stress-strain response may lead to an unstable model, and 
there is an option to check this to a certain tolerance level, see dimensionless parameter 
STOL.    The  check  is  done  by  examining  the  eigenvalues  of  the  tangent  modulus  at 
selected stretch points and a  warning message is issued if an eigenvalue is less than –
STOL × BULK, where BULK indicates the bulk modulus of the material.  For STOL < 0 
the  check  is  disabled,  otherwise  it  should  be  chosen  with  care,  a  too  small  value  may 
detect instabilities that are insignificant in practice.  To avoid significant instabilities it is 
recommended  to  use  smooth  curves,  at  best  the  curves  should  be  continuously 
differentiable,  in  fact  for  the  incompressible  case,  a  sufficient  condition  for  stability  is 
that the stress-stretch curve 𝑆(𝜆) can be written as 
𝑆(𝜆) = 𝐻(𝜆) −
⎜⎛ 1
⎟⎞
√𝜆⎠
⎝
𝜆√𝜆
where 𝐻(𝜆) is a function with 𝐻(1) = 0 and 𝐻′(𝜆) > 0. 
Rate  effects  are  taken  into  account  through  linear  viscoelasticity  by  a  convolution 
integral of the form: 
𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)
∂𝜀𝑘𝑙
∂𝜏
𝑑𝜏 
or in terms of the second Piola-Kirchhoff stress, {𝑆0 }, and Green's strain tensor, {𝑆RT},
𝑆𝑖𝑗 = ∫ 𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏)
∂𝐸𝑘𝑙
∂𝜏
𝑑𝜏
where  𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)  and  𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏)  are  the  relaxation  functions  for  the  different  stress 
measures.    This  stress  is  added  to  the  stress  tensor  determined  from  the  strain  energy 
functional. 
If we wish to include only simple rate effects, the relaxation function is represented by 
six terms from the Prony series: 
given by, 
𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚𝑒−𝛽𝑡
𝑚=1
𝑔(𝑡) = ∑ 𝐺𝑖𝑒−𝛽𝑖𝑡
𝑖=1
This  model  is  effectively  a  Maxwell  fluid  which  consists  of  a  dampers  and  springs  in 
series.    We  characterize  this  in  the  input  by  shear  moduli, 𝐺𝑖,  and  decay  constants, 𝛽𝑖.  
The viscoelastic behavior is optional and an arbitrary number of terms may be used. 
For VFLAG = 1, the viscoelastic term is 
𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)
∂𝜎𝑘𝑙
∂𝜏
𝑑𝜏 
𝐸  is the instantaneous stress evaluated from the internal energy functional.  The 
where 𝜎𝑘𝑙
coefficients  in  the  Prony  series  therefore  correspond  to  normalized  relaxation  moduli 
instead of elastic moduli. 
The Mooney-Rivlin rubber model (model 27) is obtained by specifying n = 1.  In spite of 
the  differences  in  formulations  with  model  27,  we  find  that  the  results  obtained  with 
this  model  are  nearly  identical  with  those  of  material  27  as  long  as  large  values  of 
Poisson’s ratio are used.
*MAT_SIMPLIFIED_RUBBER_WITH_DAMAGE 
An available options includes: 
LOG_LOG_INTERPOLATION 
This  is  Material  Type  183.    This  material  model  provides  an  incompressible  rubber 
model defined by a  single uniaxial load curve for loading (or a table if rate effects are 
considered)  and  a  single  uniaxial  load  curve  for  unloading.    This  model  is  similar  to 
*MAT_SIMPLIFIED_RUB-BER/FOAM  This  material  may  be  used  with  both  shell  and 
solid elements. 
This  material 
collaboration with Paul Du Bois, LSTC, and Prof.  Dave J.  Benson, UCSD. 
law  has  been  developed  at  DaimlerChrysler,  Sindelfingen, 
in 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
K 
F 
3 
4 
MU 
F 
4 
5 
G 
F 
5 
6 
7 
8 
SIGF 
F 
6 
7 
8 
Variable 
SGL 
SW 
ST 
LC / TBID TENSION 
RTYPE 
AVGOPT 
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
8 
Variable 
LCUNLD 
REF 
STOL 
Type 
F 
F 
F 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density
*MAT_SIMPLIFIED_RUBBER_WITH_DAMAGE 
DESCRIPTION
K 
MU 
G 
SIGF 
SGL 
SW 
ST 
LC/TBID 
Linear bulk modulus. 
Damping coefficient. 
Shear  modulus  for  frequency  independent  damping.    Frequency
independent  damping  is  based  of  a  spring  and  slider  in  series.
The critical stress for the slider mechanism is SIGF defined below.
For  the  best  results,  the  value  of  G  should  be  250-1000  times 
greater than SIGF. 
Limit stress for frequency independent, frictional, damping. 
Specimen gauge length 
Specimen width 
Specimen thickness 
Load  curve  or  table  ID,  see  *DEFINE_TABLE,  defining  the  force 
versus actual change in the gauge length.  If SGL, SW, and ST are
set to unity (1.0), then curve LC is also engineering stress versus
engineering  strain.    If  the  table  definition  is  used  a  family  of
curves  are  defined  for  discrete  strain  rates.    The  load  curves 
should  cover  the  complete  range  of  expected  loading,  i.e.,  the
smallest stretch ratio to the largest. 
TENSION 
Parameter  that  controls  how  the  rate  effects  are  treated.
Applicable to the table definition. 
EQ.-1.0: rate  effects  are  considered  during 
tension  and 
compression loading, but not during unloading, 
EQ.0.0:  rate  effects  are  considered  for  compressive  loading
only, 
EQ.1.0:  rate  effects  are  treated  identically  in  tension  and
compression. 
RTYPE 
Strain rate type if a table is defined: 
EQ.0.0: true strain rate, 
EQ.1.0: engineering strain rate
VARIABLE   
AVGOPT 
LCUNLD 
DESCRIPTION
Averaging  option  determine  strain  rate  to  reduce  numerical
noise. 
EQ.0.0: simple average of twelve time steps, 
EQ.1.0: running 12 point average. 
Load  curve,  see  *DEFINE_CURVE,  defining  the  force  versus 
actual change in the gauge length during unloading.  The unload
curve  should  cover  exactly  the  same  range  as  LC  (or  as  the  first
curve  of  table  TBID)  and  its  end  points  should  have  identical
values,  i.e.,  the  combination  of  LC  (or  as  the  first  curve  of  table 
TBID)  and  LCUNLD  describes  a  complete  cycle  of  loading  and
unloading. 
REF 
Use  reference  geometry  to  initialize  the  stress  tensor.    The
reference geometry is defined by the keyword:*INITIAL_FOAM_-
REFERENCE_GEOMETRY . 
EQ.0.0: off, 
EQ.1.0: on. 
STOL 
Tolerance in stability check, see remark 2. 
Remarks: 
1.  The  LOG_LOG_INTERPOLATION  option  interpolates  the  strain  rate  effect  in 
the table TBID using log-log interpolation. 
2.  Bad  choice  of  curves  for  the  stress-strain  response  may  lead  to  an  unstable 
model,  and  there  is  an  option  to  check  this  to  a  certain  tolerance  level,  see  di-
mensionless parameter STOL.  The check is done by examining the eigenvalues 
of  the  tangent  modulus  at  selected  stretch  points  and  a  warning  message  is 
issued if an eigenvalue is less than –STOL × BULK, where BULK indicates the 
bulk modulus of the material.  For STOL < 0 the check is disabled, otherwise it 
should  be  chosen  with  care,  a  too  small  value  may  detect  instabilities  that  are 
insignificant in practice.  To avoid significant instabilities it is recommended to 
use smooth curves, at best the curves should be continuously differentiable, in 
fact  for  the  incompressible  case,  a  sufficient  condition  for  stability  is  that  the 
stress-stretch curve 𝑆(𝜆) can be written as 
𝑆(𝜆) = 𝐻(𝜆) −
)
𝐻( 1
√𝜆
𝜆√𝜆
where 𝐻(𝜆) is a function with 𝐻(1) = 0 and 𝐻′(𝜆) > 0.
*MAT_184 
This  is  Material  Type  184.    It  is  a  simple  cohesive  elastic  model  for  use  with  cohesive 
element  fomulations;  see  the  variable  ELFORM  in  *SECTION_SOLID  and  *SECTION_
SHELL. 
  Card 1 
1 
2 
3 
4 
Variable 
MID 
RO 
ROFLG 
INTFAIL 
Type 
A8 
F 
F 
F 
5 
ET 
F 
6 
7 
8 
EN 
FN_FAIL 
FT_FAIL 
F 
F 
F 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density 
ROFLG 
INTFAIL 
ET 
EN 
Flag  for  whether  density  is  specified  per  unit  area  or  volume.
ROFLG = 0  specified  density  per  unit  volume  (default),  and
ROFLG = 1  specifies  the  density  is  per  unit  area  for  controlling
the mass of cohesive elements with an initial volume of zero. 
The  number  of  integration  points  required  for  the  cohesive
element to be deleted.  If it is zero, the element won’t be deleted
even if it satisfies the failure criterion.  The value of INTFAIL may
range from 1 to 4, with 1 the recommended value. 
The stiffness in the plane of the cohesive element. 
The stiffness normal to the plane of the cohesive element. 
FN_FAIL 
The traction in the normal direction for tensile failure. 
FT_FAIL 
The traction in the tangential direction for shear failure. 
Remarks: 
This material cohesive model outputs three tractions having units of force per unit area 
into the d3plot database rather than the usual six stress components.  The in plane shear 
traction along the 1-2 edge replaces the 𝑥-stress, the orthogonal in plane shear traction 
replaces the 𝑦-stress, and the traction in the normal direction replaces the 𝑧-stress.
*MAT_COHESIVE_TH 
This is Material Type 185.  It is a cohesive model by Tvergaard and Hutchinson [1992] 
in 
for  use  with  cohesive  element 
*SECTION_SOLID  and  *SECTION_SHELL.    The  implementation  is  based  on  the 
description  of  the  implementation  in  the  Sandia  National  Laboratory  code,  Tahoe 
[2003]. 
the  variable  ELFORM 
fomulations;  see 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
RO 
ROFLG 
INTFAIL 
SIGMAX 
NLS 
TLS 
Type 
A8 
  Card 2 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
8 
Variable 
LAMDA1  LAMDA2 
LAMDAF 
STFSF 
Type 
F 
F 
F 
F 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density 
ROFLG 
INTFAIL 
Flag  for  whether  density  is  specified  per  unit  area  or  volume.
ROFLG = 0  specified  density  per  unit  volume  (default),  and
ROFLG = 1  specifies  the  density  is  per  unit  area  for  controlling
the mass of cohesive elements with an initial volume of zero. 
The  number  of  integration  points  required  for  the  cohesive
element to be deleted.  If it is zero, the element won’t be deleted
even if it satisfies the failure criterion.  The value of INTFAIL may
range from 1 to 4, with 1 the recommended value. 
SIGMAX 
Peak traction. 
NLS 
TLS 
2-974 (EOS) 
Length scale (maximum separation) in the normal direction.
(
)
t λ
max
reversible 
loading/unloadin
g 
λ λ
/
fail
3 
2 
Λ Λ
1/
fail
Λ Λ
2/
fail
Figure M185-1.  Relative displacement and trilinear traction-separation law 
  VARIABLE   
DESCRIPTION
LAMDA1 
Scaled distance to peak traction (Λ1). 
LAMDA2 
Scaled distance to beginning of softening (Λ2). 
LAMDAF 
Scaled distance for failure (Λfail). 
STFSF 
Penetration  stiffness  multiplier.    The  penetration  stiffness,  PS,  in 
terms of input parameters becomes: 
PS =
STFSF × SIGMAX
NLS × (LAMDA1
LAMDAF
)
Remarks: 
In  this  cohesive  material  model,  a  dimensionless  separation  measure  λ  is  used,  which 
grasps  for  the  interaction  between  relative  displacements  in  normal  (δ3  -  mode  I)  and 
tangential (δ1, δ2 - mode II) directions : 
𝜆 = √(
𝛿1
TLS
)
+ (
𝛿2
TLS
)
+ (
)
⟨𝛿3⟩
NLS
where  the  Mc-Cauley  bracket  is  used  to  distinguish  between  tension  (δ3≥0)  and 
compression  (δ3 < 0).  NLS  and  TLS  are  critical  values,  representing  the  maximum 
separations in the interface in normal and tangential direction.  For stress calculation, a 
trilinear traction-separation law is used, which is given by :
𝑡(𝜆) =
𝜎max
⎧
{
{
{
⎨
{
{
{
⎩
𝜎max
𝜎max
Λ1/Λfail
1 − 𝜆
1 − Λ2/Λfail
𝜆 < Λ1/Λfail
Λ1/Λfail < 𝜆 < Λ2/Λfail
Λ2/Λfail < 𝜆 < 1
With  these  definitions,  the  traction  drops  to  zero  when  𝜆 = 1.    Then,  a  potential  𝜙  is 
defined as: 
𝜙(𝛿1, 𝛿2, 𝛿3) = NLS ×   ∫ 𝑡(𝜆̅̅̅̅)
 𝑑𝜆̅̅̅̅ 
Finally, tangential components (t1, t2) and  normal component (t3) of the traction acting 
on the interface in the fracture process zone are given by: 
𝑡1,2 =
∂𝜙
∂𝛿1,2
=
𝑡(𝜆)
𝛿1,2
TLS
NLS
TLS
,      𝑡3 =
∂𝜙
∂𝛿3
=
𝑡(𝜆)
𝛿3
NLS
which in matrix notation is 
NLS
TLS2
⎤
⎥
⎥
⎥
⎥
⎥
⎥
NLS⎦
In case of compression (𝛿3 < 0), penetration is avoided by: 
𝑡1
⎤ =
⎡
𝑡2
⎥
⎢
𝑡3⎦
⎣
NLS
TLS2
𝑡(𝜆)
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎣
𝛿1
⎤
⎡
𝛿2
⎥
⎢
𝛿3⎦
⎣
𝑡3 =
STFSF × 𝜎max
NLS × Λ1/Λfail
𝛿3 
Loading and unloading follows the same path, i.e.  this model is completely reversible. 
This cohesive material model outputs three tractions having units of force per unit area 
into  the  D3PLOT  database  rather  than  the  usual  six  stress  components.    The  in  plane 
shear traction t1 along the 1-2 edge replaces the x-stress, the orthogonal in plane shear 
traction t2 replaces the y-stress, and the traction in the normal direction t3  replaces the z-
stress.
*MAT_186 
includes 
three  general 
This is Material Type 186 and can be used only with cohesive element fomulations; see 
the  variable  ELFORM  in  *SECTION_SOLID  and  *SECTION_SHELL.  The  material 
model 
interaction  cohesive 
formulations  with  arbitrary  normalized  traction-separation  law  given  by  a  load  curve 
(TSLC).  These three formulations are differentiated via the type of effective separation 
parameter  (TES).  The  interaction  between  fracture  modes  I  and  II  is  considered,  and 
irreversible  conditions  are  enforced  via  a  damage  formulation  (unloading/reloading 
path pointing to/from the origin). See remarks for details. 
irreversible  mixed-mode 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
RO 
ROFLG 
INTFAIL 
TES 
TSLC 
GIC 
GIIC 
Type 
A8 
  Card 2 
1 
Variable 
XMU 
Type 
F 
  VARIABLE   
MID 
F 
2 
T 
F 
F 
3 
S 
F 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
STFSF 
TSLC2 
F 
F 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density. 
ROFLG 
INTFAIL 
Flag  for  whether  density  is  specified  per  unit  area  or  volume.
ROFLG = 0  specifies  density  per  unit  volume  (default),  and
ROFLG = 1  specifies  the  density  is  per  unit  area  for  controlling
the mass of cohesive elements with an initial volume of zero. 
Number  of  integration  points  required  for  a  cohesive  element  to
be deleted.  If it is zero, the element will not be deleted even if it
satisfies failure criterion.  The value of INTFAIL may range from
1 to 4, with 1 the recommended value.
⁄
𝑡max
1.0 
*MAT_COHESIVE_GENERAL 
Possible shape of TSLC
𝐴TSLC
𝜆 =
𝛿F 
Mode I  Mode II
𝑡max 
𝑇 
𝑆 
𝛿F 
𝐺C 
𝐺I
𝐴TSLC𝑇
𝐺II
𝐴TSLC𝑆
C 
𝐺I
C 
𝐺II
𝜆0
1.0 
Figure M186-1.  Normalized traction-separation law 
  VARIABLE   
DESCRIPTION
TES 
Type of effective separation parameter (ESP). 
EQ.0.0 or 1.0:  a  dimensional  separation  measure  is  used.    For
the interaction between mode I and II, a mixed-
mode  propagation  criterion 
  For
TES = 0.0  this  is  a  power-law,  and  for  TES = 1.0 
this  is  the  Benzeggagh-Kenane  law  [1996].    See 
remarks below. 
is  used. 
EQ.2.0: 
a  dimensionless  separation  measure  is  used, 
which grasps for the interaction between mode I
displacements and mode II displacements (simi-
lar  to  MAT_185,  but  with  damage  and  general 
traction-separation law).  See remarks below. 
Normalized traction-separation load curve ID. The curve must be 
normalized  in  both  coordinates  and  must  contain  at  least  three
points:  (0.0, 0.0),  (𝜆0, 1.0),  and  (1.0, 0.0),  which  represents  the 
origin, the peak and the complete failure, respectively .  A platform can exist in the curve like the tri-linear TSLC 
. 
Fracture toughness / energy release rate 𝐺𝐼
𝑐 for mode I 
Fracture toughness / energy release rate 𝐺𝐼𝐼
𝑐  for mode II 
Exponent that appears in the power failure criterion (TES = 0.0) or 
(TES = 1.0). 
the 
Recommended values for XMU are between 1.0 and 2.0. 
Benzeggagh-Kenane 
criterion 
failure 
TSLC 
GIC 
GIIC 
XMU 
T 
Peak traction in normal direction (mode I)
VARIABLE   
DESCRIPTION
S 
Peak traction in tangential direction (mode II) 
Penetration  stiffness  multiplier  for  compression.  Factor = (1.0 +
STFSF) is used to scale the compressive stiffness, i.e.  no scaling is
done with STFSF = 0.0 (recommended). 
Normalized  traction-separation  load  curve  ID  for  Mode  II.  The 
curve  must  be  normalized  in  both  coordinates  and  must  contain
at  least  three  points:  (0.0, 0.0),  (𝜆0, 1.0),  and  (1.0, 0.0),  which 
represents  the  origin,  the  peak  and  the  complete  failure,
respectively  .    If  not  specified,  TSLC  is  used 
for Mode II behavior as well. 
STFSF 
TSLC2 
Remarks: 
All  three  formulations  have  in  common  that  the  traction-separation  behavior  of  this 
𝑐  and S for tangential mode II 
𝑐 and T for normal mode I, 𝐺𝐼𝐼
model is mainly given by 𝐺𝐼
and an arbitrary normalized traction-separation load curve for both modes .  The maximum (or failure) separations are then given by: 
𝐹 =
𝛿𝐼
𝐺𝐼
𝐴TSLC × T
  ,    𝛿𝐼𝐼
𝐹 =
𝐺𝐼𝐼
𝐴TSLC × S
where  𝐴𝑇𝑆𝐿𝐶  is  the  area  under  the  normalized  traction-separation  curve  given  with 
TSLC. 
If TSLC2 is defined 
𝐹 =
𝛿𝐼
𝐺𝐼
𝐴TSLC × T
  ,    𝛿𝐼𝐼
𝐹 =
𝐺𝐼𝐼
𝐴TSLC2 × S
Where  𝐴𝑇𝑆𝐿𝐶2  is  the  area  under  the  normalized  traction-separation  curve  given  with 
TSLC2.
traction
3 
2 
1 
Fδ
II
II
Figure M186-2.  Mixed mode traction-separation law 
First and second formulation (TES = 0.0 and TES = 1.0): 
For  mixed-mode  behavior,  three  different  formulations  are  possible  (where  default 
TES = 0.0  with  XMU = 1.0  is  recommended  as a  first  try).    Here,  the  total  mixed-mode 
2 , where 𝛿𝐼 = 𝛿3 is the separation in 
2 + 𝛿𝐼𝐼
relative displacement 𝛿𝑚 is defined as 𝛿𝑚 = √𝛿𝐼
2  is  the  separation  in  tangential  direction 
2 + 𝛿2
normal  direction  (mode  I)  and  𝛿𝐼𝐼 = √𝛿1
(mode II).  See Figure M186-2.  The ultimate mixed-mode displacement 𝛿𝐹 (total failure) 
for the power law (TES = 0.0) is: 
𝛿𝐹 =
1 + 𝛽2
⎡(
⎢
𝐴TSLC ⎣
𝑐)
𝐺𝐼
XMU
+ (
S × 𝛽2
𝐺𝐼𝐼
𝑐 )
XMU
XMU
−   1
⎤
⎥
⎦
If TSLC2 is defined this changes to: 
𝛿𝐹 = 1 + 𝛽2
𝐴TSLC × T
𝐺𝐼
⎡(
⎢
⎣
XMU
)
+ (
𝐴TSLC2 × S × 𝛽2
𝐺𝐼𝐼
)
XMU
XMU
−   1
⎤
⎥
⎦
and alternatively for the Benzeggagh-Kenane law [1996]  (TES = 1.0): 
𝛿𝐹 =
1 + 𝛽2
⎡𝐺𝐼
⎢
𝐴TSLC(T + S × 𝛽2) ⎣
𝑐 + (𝐺𝐼𝐼
𝑐 − 𝐺𝐼
𝑐) (
XMU
S × 𝛽2
𝑇 + S × 𝛽2)
⎤ 
⎥
⎦
If TSLC2 is defined this changes to: 
𝛿𝐹 =
1 + 𝛽2
𝐴TSLC × T + 𝐴TSLC2 × S × 𝛽2
𝑐 + (𝐺𝐼𝐼
𝑐 − 𝐺𝐼
𝑐) (
⎡𝐺𝐼
⎢
⎣
𝐴TSLC2 × S × 𝛽2
𝐴TSLC × 𝑇 + 𝐴TSLC2 × S × 𝛽2)
XMU
⎤ 
⎥
⎦
where  𝛽 = 𝛿𝐼𝐼/𝛿𝐼  is  the  “mode  mixity”.    The  larger  the  exponent  XMU  is  chosen,  the 
larger the fracture toughness in mixed-mode situations will be.  In this model, damage 
  irreversible  conditions  are  enforced  with 
of  the  interface  is  considered,  i.e. 
loading/unloading  paths  coming  from/pointing  to  the  origin.    This  formulation  is 
similar  to  MAT_COHESIVE_MIXED_MODE  (MAT_138),  but  with  the  arbitrary 
traction-separation law TSLC. 
Third formulation (TES = 2.0): 
Here,  a  dimensionless  effective  separation  parameter  𝜆  is  used,  which  grasps  for  the 
interaction between relative displacements in normal (𝛿3 - mode I) and tangential (𝛿1,𝛿2 
- mode II) directions: 
𝜆 =
√
√√
⎷
 (
𝛿1
𝐹 )
𝛿𝐼𝐼
+ (
𝛿2
𝐹 )
𝛿𝐼𝐼
+ ⟨
𝛿3
𝐹⟩
𝛿𝐼
𝐹  and  𝛿𝐼𝐼
where  the  Mc-Cauley  bracket  is  used  to  distinguish  between  tension  (𝛿3 ≥ 0)  and 
𝐹   are  critical  values,  representing  the  maximum 
compression  (𝛿3 < 0).  𝛿𝐼
separations in the interface in normal and tangential direction .  For stress calculation, 
the  normalized  traction-separation  load  curve  TSLC  is  used:  𝑡 = 𝑡max × 𝑡 ̅(𝜆).    This 
formulation  is  similar  to  MAT_COHESIVE_TH  (MAT_185),  but  with  the  arbitrary 
traction-separation  law  and  a  damage  formulation  (i.e.    irreversible  conditions  are 
enforced with loading/unloading paths coming from/pointing to the orig
*MAT_SAMP-1 
Purpose: This is Material Type 187 (Semi-Analytical Model for Polymers).  This material 
model uses an isotropic C-1 smooth yield surface for the description of non-reinforced 
plastics.  Details of the implementation are given in [Kolling, Haufe, Feucht and Du Bois 
2005]. 
This  material 
collaboration with Paul Du Bois and Dynamore, Stuttgart. 
law  has  been  developed  at  DaimlerChrysler,  Sindelfingen, 
in 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
4 
5 
6 
7 
8 
BULK 
GMOD 
EMOD 
NUE 
RBCFAC  NUMINT 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
8 
Variable 
LCID-T 
LCID-C 
LCID-S 
LCID-B 
NUEP 
LCID-P 
INCDAM 
Type 
I 
  Card 3 
1 
I 
2 
I 
3 
I 
4 
F 
5 
I 
6 
7 
8 
Variable 
LCID-D 
EPFAIL 
DEPRPT  LCID_TRI
LCID_LC 
Type 
I 
  Card 4 
1 
F 
2 
F 
3 
I 
4 
I 
5 
6 
7 
8 
Variable 
MITER 
MIPS 
INCFAIL 
ICONV 
ASAF 
Type 
I 
I 
I 
I
*MAT_SAMP-1 
Optional Card. 
*MAT_187 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCEMOD 
BETA 
FILT 
Type 
F 
F 
F 
  VARIABLE   
MID 
DESCRIPTION
Material identification. A unique number or label not exceeding 8 
characters must be specified. 
RO 
Mass density 
BULK 
Bulk modulus, used by LS-DYNA in the time step calculation 
GMOD 
Shear modulus, used by LS-DYNA in the time step calculation 
EMOD 
Young’s modulus 
NUE 
Poisson ratio
qs 
t 
qbt 
linear 
extrapolation 
qc 
qbc 
rbcfac > 
1 
rbcfac = 1 
rbcfac < 1 
rbcfac = 0.5 
(lower bound)
von Mises stress 
pressure  
required 
input 
optional 
input 
biaxial tension 
bt 
tension 
t 
shear 
s 
compression 
c 
bc  biaxial compression 
q 
p 
data 
data 
rbcfac = 
qbc 
qc 
extrapolated data 
Figure M187-1.  von Mises stress as a function of pressure 
  VARIABLE   
RBCFAC 
DESCRIPTION
Ratio  of  yield  in  biaxial  compression  vs.    yield  in  uniaxial
compression.  If RBCFAC is nonzero and all four curves LCID-T, 
LCID-C,  LCID-S,  and  LCID-B  are  defined,  a  piecewise-linear 
yield surface as shown in Figure M187-1 is activated.  See Remark 
3.  Default is 0. 
NUMINT 
Number of integration points which must fail before the element
is deleted.  This option is available for shells and solids. 
LT.0.0: |NUMINT|  is  percentage  of  integration  points/layers 
which must fail before shell element fails.  For fully in-
tegrated  shells,  a  methodology  is  used  where  a  layer 
fails  if  one  integration  point  fails  and  then  the  given
percentage  of  layers  must  fail  before  the  element  fails.
Only available for shells.
*MAT_SAMP-1 
  VARIABLE   
LCID-T 
LCID-C 
LCID-S 
LCID-B 
NUEP 
LCID-P 
*MAT_187 
DESCRIPTION
Load  curve  or  table  ID  giving  the  yield  stress  as  a  function  of
plastic  strain,  these  curves  should  be  obtained  from  quasi-static 
and  (optionally)  dynamic  uniaxial  tensile  tests,  this  input  is
mandatory  and  the  material  model  will  not  work  unless  at  least
one tensile stress-strain curve is given.  If LCID-T is a table ID, the 
table  values  are  plastic  strain  rates,  and  a  curve  of  yield  stress
versus  plastic  strain  must  be  given  for  each of  those  strain rates.
If  the  first  value  in  the  table  is  negative,  LS-DYNA  assumes  that 
all  the  table  values  represent  the  natural  logarithm  of  plastic 
strain rate. When the highest plastic strain rate is several orders of
magnitude greater than the lowest strain rate, it is recommended
that the natural log of plastic strain rate be input in the table.  See 
Remark 4. 
Load  curve  ID  giving  the  yield  stress  as  a  function  of  plastic
strain,  this  curve  should  be  obtained  from  a  quasi-static  uniaxial 
compression test, this input is optional. 
Load  curve  ID  giving  the  yield  stress  as  a  function  of  plastic 
strain, this curve should be obtained from a quasi-static shear test, 
this input is optional. 
Load  curve  ID  giving  the  yield  stress  as  a  function  of  plastic
strain,  this  curve  should  be  obtained  from  a  quasi-static  biaxial 
tensile test, this input is optional. 
Plastic  Poisson’s  ratio:  an  estimated  ratio  of  transversal  to
longitudinal  plastic  rate  of  deformation  under  uniaxial  loading
should be given. 
Load  curve  ID  giving  the  plastic  Poisson's  ratio  as  a  function  of
plastic  strain  during  uniaxial  tensile  and  uniaxial  compressive
testing.    The  plastic  strain  on  the  abscissa  is  negative  for
compression  and  positive  for  tension.        It  is  important  to  cover
both  tension  and  compression.    If  LCID-P  is  given,  the  constant 
value of plastic Poisson's ratio NUEP is ignored. 
INCDAM 
Flag to control the damage evolution as a function of triaxiality. 
EQ.0: damage evolution is independent of the triaxialty. 
EQ.1: an  incremental  formulation  is  used  to  compute  the
damage.
LCID-D 
EPFAIL 
DEPRPT 
LCID_TRI 
LCID_LC 
MITER 
MIPS 
*MAT_SAMP-1 
DESCRIPTION
Load  curve  ID  giving  the  damage  parameter  as  a  function  of
equivalent  plastic  strain  during  uniaxial  tensile  testing.    By
default this option assumes that effective (i.e.  undamaged) yield
values are used in the load curves LCID-T,  LCID-C, LCID-S and 
LCID-B.  If LCID-D is given a negative value, true (i.e.  damaged)
yield stress values can be used.  In this case  an automatic stress-
strain  recalibration  (ASSR)  algorithm  is  activated.    The  damage
value  must  be  defined  in  the  range  0 ≤ 𝑑 < 1.    If  EPFAIL  and 
DEPRPT  are  given,  the  curve  is  used  only  until  the  effective
plastic strain reaches EPFAIL. 
This  parameter  is  the  equivalent  plastic  strain  at  failure.    If
EPFAIL  is  given  as  a  negative  integer,  a  load  curve  is  expected 
that  defines  EPFAIL  as  a  function  of  the  plastic  strain  rate.
Default value is 105. 
Increment  of  equivalent  plastic  strain  between  failure  point  and
rupture point.  Stresses will fade out to zero between EPFAIL and
EPFAIL+DEPRPT.    If  DEPRPT  is  given  a  negative  value  a  curve
definition is expected where DEPRPT is defined as function of the
triaxiality. 
Load  curve  that  specifies  a  factor  that  works  multiplicatively  on
the  value  of  EPFAIL  depending  on 
(i.e. 
pressure/sigma_vm).    For  a  triaxiality  of  -1/3  a  value  of  1.0 
should be specified. 
triaxiality 
the 
Load  curve  that  specifies  a  factor  that  works  multiplicatively  on
the  value  of  EPFAIL  depending  on  a  characteristic  element
length, defined as the average length of spatial diagonals. 
Maximum  number  of  iterations  in  the  cutting  plane  algorithm,
default is set to 400 
Maximum number of iterations in the secant iteration performed
to enforce plane stress (shell elements only), default set to 10 
INCFAIL 
Flag to control the failure evolution as a function of triaxiality. 
EQ.0:  Failure evolution is independent of the triaxiality. 
EQ.1:  Incremental  formulation  is  used  to  compute  the  failure
value.  
EQ.-1: the failure model is deactivated.
*MAT_SAMP-1 
LCID_C = 0
⎫
}}
LCID_S = 0
⎬
}}
LCID_B = 0⎭
⇒
⎧𝜎𝑐 = 𝜎𝑡
{{{
⎨
{{{
⎩
𝜎𝑠 =
𝜎𝑡
√3
LCID_C = 0
⎫
}}
LCID_S ≠ 0
⎬
}}
LCID_B = 0⎭
LCID_C ≠ 0
⎫
}}
LCID_S = 0
⎬
}}
LCID_B = 0⎭
⇒ 𝜎c =
√3𝜎𝑡𝜎𝑠
2𝜎𝑡 − √3𝜎𝑠
⇒ 𝜎𝑠 =
2𝜎c𝜎𝑡
√3(𝜎𝑡 + 𝜎𝑐)
LCID_C = 0
⎫
}}
LCID_S = 0
⎬
}}
LCID_B ≠ 0⎭
⇒
⎧𝜎𝑐 =
{{
⎨
{{
⎩
𝜎𝑠 =
𝜎𝑡𝜎𝑏
3𝜎𝑏 − 2𝜎𝑡
𝜎𝑡𝜎𝑏
√3(2𝜎𝑏 − 𝜎𝑡)
*MAT_187 
𝜎vM
von Misses cylinder
𝜎vM
Drucker-Prager Cone
⎫
}}}
⎬
}}}
⎭
⎫
}
}
}
}
}
}
}
}
}
}
}
}
⎬
}
}
}
}
}
}
}
}
}
}
}
}
⎭
Figure M187-2.  Fewer than 3 load curves 
  VARIABLE   
DESCRIPTION
ICONV 
Formulation flag: 
EQ.0: default 
EQ.1: yield  surface  is  internally  modified  by  increasing  the 
shear yield until a convex yield surface is achieved. 
ASAF 
Safety factor, used only if ICONV = 1, values between 1 and 2 can 
improve convergence, however the shear yield will be artificially
increased if this option is used, default is set to 1. 
LCEMOD 
Load curve ID defining Young’s modulus as function of effective
strain rate. 
BETA 
FILT 
Decay  constant  in  viscoelastic  law:  𝜎̇ (𝑡) = −β ∙ 𝜎(𝑡) + 𝐸(𝜀̇(𝑡)) ∙
𝜀̇(𝑡) 
Factor  for  strain  rate  filtering:  𝜀̇𝑛+1
𝑎𝑣𝑔 
𝜀̇𝑛
𝑎𝑣𝑔 = (1 − FILT) ∙ 𝜀̇𝑛+1
𝑐𝑢𝑟𝑟 + FILT ∙
LCID_C ≠ 0
LCID_S ≠ 0
⎫
}}
⎬
}}
LCID_B = 0⎭
⇒ normal SAMP-1 behavior
LCID_C ≠ 0
LCID_S = 0
⎫
}}
⎬
}}
LCID_B ≠ 0⎭
⇒ 𝜎𝑠 =
√3
√
3𝜎𝑏
2𝜎𝑐𝜎𝑡
(2𝜎𝑏 + 𝜎𝑐)(2𝜎𝑏 − 𝜎𝑡)
LCID_C = 0
LCID_S ≠ 0
⎫
}}
⎬
}}
LCID_B ≠ 0⎭
⇒ 𝜎𝑐 =
6(162𝜎𝑏
2𝜎𝑠
2 + 323𝜎𝑏
2 + 𝜎𝑏𝜎𝑠
2𝜎𝑡)
2𝜎𝑡 + 3𝜎𝑠
6𝜎𝑏𝜎𝑠
2𝜎𝑡
LCID_C ≠ 0
LCID_S ≠ 0
⎫
}}
⎬
}}
LCID_B ≠ 0⎭
⇒ overspecified, least  square
⎫
}
}
}
}
}
}
}
}
}
}
}
}
}
}
}
}
⎬
}
}
}
}
}
}
}
}
}
}
}
}
}
}
}
}
⎭
𝜎vM 
SAMP-1 yield surface defined 
through load curves 
Figure M187-3.  Three or more load curves 
Load curves: 
Material  SAMP-1  uses  three  yield  curves  internally  to  evaluate  a  quadratic  yield 
surface.  *MAT_SAMP-1 accepts four different kinds of yield curves, LCID_T, LCID_C, 
LCID_S,  and  LCID_B  where  data  from  tension  tests  (LCID_T)  is  always  required,  but 
the others are optional.  If fewer than three curves are defined, as indicated by setting 
the missing load curve IDs to 0, the remaining curves are generated internally. 
1.  Fewer  than  3  load  curves.    In  the  case  of  fewer  than  3  load  curves,  a  linear 
yield surface in the invariant space spanned by the pressure and the von Mises 
stress is generated using the available data.  See figure M187-2. 
2.  Three or more load curves.  See figure M187-3. 
Remarks: 
1.  Damage.    If  the  LCID_D  is  given,  then  a  damage  curve  as  a  function  of 
equivalent  plastic  strains  acting  on  the  stresses  is  defined  as  shown  in  Figure 
M187-4.
𝑑 
1.0 
𝑑𝑐 
𝜀fail
𝜀erode
𝜀𝑝
𝑝  
(cid:1526)𝜀rpt
Figure M187-4.  EPFAIL and DEPRPT defined the failure and fading behavior
of a single element. 
Since  the  damaging  curve  acts  on  the  yield  values,  the  inelastic  results  are  ef-
fected  by  the  damage  curve.    As  a  means  to  circumvent  this,  the  load  curve 
LCID-D may be given a negative ID.  This will lead to an internal conversion of 
from nominal to effective stresses (ASSR). 
2.  Unsolvable Yield Surface Case.  Since the generality of arbitrary curve inputs 
allows  unsolvable  yield  surfaces,  SAMP  may  modify  curves  internally.    This 
will  always  lead  to  warning  messages  at  the  beginning  of  the  simulation  run.  
One modification that is not allowed are negative tangents of the last two data 
points of any of the yield curves. 
3.  RBCFAC.    If  RBCFAC  is  nonzero  and  curves  LCID-T,  LCID-C,  LCID-S,  and 
LCID-B  are  specified,  the  yield  surface  in  𝐼1-𝜎𝑣𝑚  -stress  space  is  constructed 
such  that  a  piecewise-linear  yield  surface  is  activated.    This  option  can  help 
promote convergence of the plasticity algorithm.  Figure M187-1 illustrates the 
effect of RBCFAC on behavior in biaxial compression.  
4.  Dynamic Amplification Factor for Yield Stress.  If LCID-T is given as a table 
specifying strain-rate scaling of the yield stress, then the compressive, shear and 
biaxial yield stresses are computed by multiplying their respective static values 
by  dynamic  amplification  factor  (dynamic/static  ratio)  of  the  tensile  yield 
stress.
*MAT_SAMP-1 
# 
2 
3 
4 
5 
6 
Interpretation 
plastic strain in tension/compression 
plastic strain in shear 
biaxial plastic strain 
damage 
volumetric plastic strain 
16  plastic strain rate in tension/compression 
17  plastic strain rate in shear 
18 
biaxial plastic strain rate
*MAT_THERMO_ELASTO_VISCOPLASTIC_CREEP 
This  is Material  Type 188.    In this  model,  creep  is  described  separately  from  plasticity 
using Garafalo’s steady-state hyperbolic sine creep law or Norton’s power law.  Viscous 
effects of plastic strain rate are considered using the Cowper-Symonds model.  Young’s 
modulus,  Poisson’s  ratio,  thermal  expansion  coefficient,  yield  stress,  material 
parameters  of  Cowper-Symonds  model  as  well  as  the  isotropic  and  kinematic 
hardening parameters are all assumed to be temperature dependent.  Application scope 
includes:  simulation  of  solder  joints  in  electronic  packaging,  modeling  of  tube  brazing 
process, creep age forming, etc. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
E 
F 
3 
4 
PR 
F 
4 
5 
6 
7 
8 
SIGY 
ALPHA 
LCSS 
REFTEM 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
QR1 
CR1 
QR2 
CR2 
QX1 
CX1 
QX2 
CX2 
Type 
F 
  Card 3 
Variable 
Type 
1 
C 
F 
  Card 4 
1 
F 
2 
P 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
LCE 
LCPR 
LCSIGY 
LCQR 
LCQX 
LCALPH 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
LCC 
LCP 
LCCR 
LCCX 
CRPA 
CRPB 
CRPQ 
CRPM 
Type 
F 
F 
F 
F 
F 
F 
F
*MAT_THERMO_ELASTO_VISCOPLASTIC_CREEP 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CRPLAW 
Type 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus 
Poisson’s ratio 
SIGY 
Initial yield stress 
ALPHA 
Thermal expansion coefficient 
LCSS 
Load  curve  ID  or  Table  ID.    The  load  curve  ID  defines  effective
stress versus effective plastic strain.  The table ID defines for each
temperature  value  a  load  curve  ID  giving  the  stress  versus
effective  plastic  strain  for  that  temperature.    The  stress  versus 
effective plastic strain curve for the lowest value of temperature is
used  if  the  temperature  falls  below  the  minimum  value.
Likewise,  the  stress  versus  effective  plastic  strain  curve  for  the
highest  value  of  temperature  is  used  if  the  temperature  exceeds 
the maximum value.  Card 2 is ignored with this option.   
REFTEM 
Reference temperature that defines thermal expansion coefficient
QR1 
CR1 
QR2 
CR2 
QX1 
CX1 
Isotropic hardening parameter 𝑄𝑟1 
Isotropic hardening parameter 𝐶𝑟1 
Isotropic hardening parameter 𝑄𝑟2 
Isotropic hardening parameter 𝐶𝑟2 
Kinematic hardening parameter 𝑄𝜒1 
Kinematic hardening parameter 𝐶𝜒1
VARIABLE   
DESCRIPTION
QX2 
CX2 
C 
P 
LCE 
Kinematic hardening parameter 𝑄𝜒2 
Kinematic hardening parameter 𝐶𝜒2 
Viscous material parameter 𝐶 
Viscous material parameter 𝑃 
Load  curve  for  scaling  Young's  modulus  as  a  function  of
temperature 
LCPR 
Load curve for scaling Poisson's ratio as a function of temperature
LCSIGY 
LCQR 
LCQX 
LCALPH 
LCC 
LCP 
LCCR 
LCCX 
Load  curve  for  scaling  initial  yield  stress  as  a  function  of
temperature 
Load  curve  for  scaling  the  isotropic  hardening  parameters  QR1
and QR2  or the stress given by the load curve LCSS as a function
of temperature 
Load  curve  for  scaling  the  kinematic  hardening  parameters  QX1
and QX2 as a function of temperature 
Load  curve  for  scaling  the  thermal  expansion  coefficient  as  a
function of temperature 
Load  curve  for  scaling  the  viscous  material  parameter  𝐶  as  a 
function of temperature 
Load  curve  for  scaling  the  viscous  material  parameter  𝑃  as  a 
function of temperature 
Load  curve  for  scaling  the  isotropic  hardening  parameters  CR1
and CR2  as a function of temperature 
Load  curve  for  scaling  the  kinematic  hardening  parameters  CX1
and CX2 as a function of temperature 
CRPA 
Creep law parameter 𝐴 
GT.0.0: Constant value 
LT.0.0:  Load curve ID = (-CRPA) which defines 𝐴 as a function 
of temperature, 𝐴(𝑇).
*MAT_THERMO_ELASTO_VISCOPLASTIC_CREEP 
DESCRIPTION
CRPB 
Creep law parameter 𝐵 
GT.0.0: Constant value 
LT.0.0:  Load curve ID = (-CRPB) which defines 𝐵 as a function 
of temperature, 𝐵(𝑇). 
CRPQ 
Creep  law  parameter  𝑄 = 𝐸/𝑅  where  E  is  the  activation  energy 
and R is the universal gas constant. 
GT.0.0: Constant value 
LT.0.0:  Load curve ID = (-CRPQ) which defines 𝑄 as a function 
of temperature, 𝑄(𝑇). 
CRPM 
Creep law parameter m 
GT.0.0: Constant value 
LT.0.0:  Load  curve  ID = (-CRPM)  which  defines  m  as  a 
function of temperature, 𝑚(𝑇). 
CRPLAW 
Creep law definition : 
EQ.0.0: Garofalo’s hyperbolic sine law (default). 
EQ.1.0: Norton’s power law. 
Remarks: 
If LCSS is not given any value the uniaxial stress-strain curve has the form 
𝑝 )]
𝑝 )] + 𝑄𝑟2[1 − exp(−𝐶𝑟2𝜀eff
𝑝 )] + 𝑄𝜒2[1 − exp(−𝐶𝜒2𝜀eff
𝑝 ) = 𝜎0 + 𝑄𝑟1[1 − exp(−𝐶𝑟1𝜀eff
+ 𝑄𝜒1[1 − exp(−𝐶𝜒1𝜀eff
𝜎(𝜀eff
𝑝 )]. 
Viscous  effects  are  accounted  for  using  the  Cowper-Symonds  model,  which  scales  the 
yield stress with the factor: 
𝜀̇eff
⎟⎞
𝐶 ⎠
For  CRPLAW = 0,  the  steady-state  creep  strain  rate  of  Garafalo’s  hyperbolic  sine 
equation is given by 
⎜⎛
⎝
1 +
. 
𝑝⁄
𝜀̇𝑐 = 𝐴[sinh(𝐵𝜏𝑒)]𝑚exp (−
).
For  CRPLAW = 1,  the  steady-state  creep  strain  rate  is  given  by  Norton’s  power  law 
equation: 
𝜀̇𝑐 = 𝐴(𝜏𝑒)𝐵𝑡𝑚. 
In the above, 𝜏𝑒 is the effective elastic stress in the von Mises sense, T is the temperature 
and t is the time.  The following is a schematic overview of the resulting stress update.  
The multiaxial creep strain increment is given by 
Δ𝜀𝑐 = Δ𝜀𝑐 3𝝉 𝑒
2𝜏𝑒 
where 𝛕𝑒 is the elastic deviatoric stress tensor.  Similarily the plastic and thermal strain 
increments are given by 
Δ𝜺p = Δ𝜀𝑝 3𝝉 𝑒
2𝜏𝑒 
𝑇 
Δ𝜺𝑇 = 𝛼𝑡+Δ𝑡(𝑇 − 𝑇ref)𝑰 − 𝜺𝑡
where  α  is  the  thermal  expansion  coefficient  (note  the  definition  compared  to  that  of 
other materials).  Adding it all together, the stress update is given by 
𝝈𝑡+Δ𝑡 = 𝑪𝑡+Δ𝑡(𝜺𝑡
𝑒 + Δ𝜺 − Δ𝜺𝑝 − Δ𝜺𝑐 − Δ𝜺𝑇) 
The  plasticity  is  isotropic  or  kinematic  but  with  a  von  Mises  yield  criterion,  the 
subscript in the equation above indicates the simulation time of evaluation.  Internally, 
this stress update requires the solution of a nonlinear equation in the effective stress, the 
viscoelastic strain increment and potentially the plastic strain increment.
*MAT_ANISOTROPIC_THERMOELASTIC 
This  is  Material  Type  189.    This  model  characterizes  elastic  materials  whose  elastic 
properties are temperature-dependent. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
4 
5 
6 
7 
8 
TA1 
TA2 
TA3 
TA4 
TA5 
TA6 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
C11 
C12 
C13 
C14 
C15 
C16 
C22 
C23 
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
C24 
C25 
C26 
C33 
C34 
C35 
C36 
C44 
Type 
F 
  Card 4 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
C45 
C46 
C55 
C56 
C66 
TGE 
TREF 
AOPT 
Type 
F 
F 
F 
F 
F 
F 
  Card 5 
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
3 
ZP 
F 
4 
A1 
F 
5 
A2 
F 
6 
A3 
F 
F 
8 
F 
7 
MACF
Card 6 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
7 
8 
BETA 
REF 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
TAi 
CIJ 
TGE 
TREF 
AOPT 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Curve  IDs  defining  the  coefficients  of  thermal  expansion  for  the
six components of strain tensor as function of temperature. 
Curve  IDs  defining  the  6×6  symmetric  constitutive  matrix  in 
material coordinate system as function of temperature.  Note that 
1  corresponds  to  the  a  material  direction,  2  to  the  b  material 
direction, and 3 to the c material direction. 
Curve ID  defining  the  structural  damping  coefficient  as  function 
of temperature. 
Reference temperature for the calculation of thermal loads or the
definition of thermal expansion coefficients. 
Material 
TIC/MAT_002 for a complete description.) 
option, 
axes 
(see  MAT_ANISOTROPIC_ELAS-
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES. 
EQ.1.0: locally orthotropic with material axes determined by a
point  in  space  and  the  global  location  of  the  element 
center; this is the a-direction. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by 
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the
*MAT_ANISOTROPIC_THERMOELASTIC 
DESCRIPTION
element normal. 
EQ.4.0: locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector  v,  and 
an originating point, P, which define the centerline ax-
is. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
XP, YP, ZP 
XP, YP, ZP define coordinates of point p for AOPT = 1 and 4. 
A1, A2, A3 
a1, a2, a3 define components of vector a for AOPT = 2. 
MACF 
Material  axis  change  flag  for  brick  elements   
D1, D2, D3 
d1, d2, d3 define components of vector d for AOPT = 2. 
V1, V2, V3 
v1, v2, v3 define components of vector v for AOPT = 3 and 4. 
BETA 
REF 
Material  angle  in  degrees  for  AOPT = 3,  may  be  overwritten  on 
the element card, see *ELEMENT_SOLID_ORTHO. 
Use  initial  geometry  to  initialize  the  stress  tensor
*MAT_FLD_3-PARAMETER_BARLAT 
This  is  Material  Type  190.    This  model  was  developed  by  Barlat  and  Lian  [1989]  for 
modeling sheets with anisotropic materials under plane stress conditions.  This material 
allows  the  use  of  the  Lankford  parameters  for  the  definition  of  the  anisotropy.    This 
particular development is due to Barlat and Lian [1989].  It has been modified to include 
a  failure  criterion  based  on  the  Forming  Limit  Diagram.    The  curve  can  be  input  as  a 
load curve, or calculated based on the n-value and sheet thickness. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
Variable 
Type 
1 
M 
F 
  Card 3 
1 
Variable 
AOPT 
Type 
F 
  Card 4 
1 
Variable 
Type 
2 
RO 
F 
2 
3 
E 
F 
3 
4 
PR 
F 
4 
5 
HR 
F 
5 
R00 
R45 
R90 
LCID 
F 
4 
I 
5 
6 
P1 
F 
6 
E0 
F 
6 
7 
P2 
F 
7 
SPI 
F 
7 
8 
ITER 
F 
8 
P3 
F 
8 
FLDCID 
RN 
RT 
FLDSAFE  FLDNIPF 
F 
7 
F 
8 
I 
F 
F 
4 
A1 
F 
5 
A2 
F 
6 
A3 
F 
F 
2 
C 
F 
2 
F 
3 
P 
F
Variable 
1 
V1 
Type 
F 
*MAT_FLD_3-PARAMETER_BARLAT 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
7 
8 
BETA 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
HR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s modulus, 𝐸 
Poisson’s ratio, 𝜈 
Hardening rule: 
EQ.1.0: linear (default) 
EQ.2.0: exponential (Swift) 
EQ.3.0: load curve 
EQ.4.0: exponential (Voce) 
EQ.5.0: exponential (Gosh) 
EQ.6.0: exponential (Hocket-Sherby) 
P1 
Material parameter: 
HR.EQ.1.0: Tangent modulus 
HR.EQ.2.0: 𝑘,  strength  coefficient 
for  Swift  exponential
hardening 
HR.EQ.4.0: 𝑎, coefficient for Voce exponential hardening 
HR.EQ.5.0: 𝑘,  strength  coefficient 
for  Gosh  exponential
hardening 
HR.EQ.6.0: 𝑎, 
coefficient 
for  Hocket-Sherby  exponential 
hardening
VARIABLE   
DESCRIPTION
P2 
Material parameter: 
HR.EQ.1.0: Yield stress 
HR.EQ.2.0: 𝑛, exponent for Swift exponential hardening 
HR.EQ.4.0: 𝑐, coefficient for Voce exponential hardening 
HR.EQ.5.0: 𝑛, exponent for Gosh exponential hardening 
HR.EQ.6.0: 𝑐, 
coefficient 
for  Hocket-Sherby  exponential 
hardening 
ITER 
Iteration flag for speed: 
ITER.EQ.0.0:  fully iterative 
ITER.EQ.1.0:  fixed at three iterations 
Generally,  ITER = 0  is  recommended.    However,  ITER = 1  is 
somewhat  faster  and  may  give  acceptable  results  in  most
problems. 
M 
R00 
R45 
R90 
LCID 
E0 
m, exponent in Barlat’s yield surface 
𝑅00, Lankford parameter determined from experiments 
𝑅45, Lankford parameter determined from experiments 
𝑅90, Lankford parameter determined from experiments 
load curve ID for the load curve hardening rule 
Material parameter 
HR.EQ.2.0: 𝜀0  for  determining  initial  yield  stress  for  Swift
exponential hardening.  (Default = 0.0) 
HR.EQ.4.0: 𝑏, coefficient for Voce exponential hardening 
HR.EQ.5.0: 𝜀0  for  determining  initial  yield  stress  for  Gosh
exponential hardening.  (Default = 0.0) 
HR.EQ.6.0: 𝑏, 
coefficient 
for  Hocket-Sherby  exponential 
hardening
*MAT_FLD_3-PARAMETER_BARLAT 
DESCRIPTION
SPI 
If 𝜀0 is zero above and HR.EQ.2.0.  (Default = 0.0) 
EQ.0.0: 𝜀0 =
⁄
(𝑛−1)
⎜⎜⎜⎛𝐸
𝑘⁄
⎝
⎟⎟⎟⎞
⎠
LE.0.2:  𝜀0 = SPI 
GT.0.2:  𝜀0 =
𝑛⁄
⎜⎜⎜⎛SPI
⁄
⎝
⎟⎟⎟⎞
⎠
P3 
Material parameter: 
HR.EQ.5.0: 𝑝, parameter for Gosh exponential hardening 
HR.EQ.6.0: 𝑛, 
exponent 
for  Hocket-Sherby 
exponential 
hardening 
AOPT 
Material axes option : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES,  and  then  rotated  about  the  shell  ele-
ment normal by the angle BETA. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by 
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the
element normal. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
C 
P 
𝐶 in Cowper-Symonds strain rate model 
𝑝 in Cowper-Symonds strain rate model, 𝑝 = 0.0 for no strain rate 
effects
VARIABLE   
FLDCID 
RN 
RT 
DESCRIPTION
Load  curve  ID  defining  the  Forming  Limit  Diagram.    Minor
engineering strains in percent are defined as abscissa values and
Major  engineering  strains  in  percent  are  defined  as  ordinate
values.  The forming limit diagram is shown in Figure M39-1.  In 
defining  the  curve  list  pairs  of  minor  and  major  strains  starting
with the left most point and ending with the right most point, see
*DEFINE_CURVE. 
Hardening  exponent  equivalent  to  the  n-value  in  a  power  law 
hardening  law.    If  the  parameter  FLDCID  is  not  defined,  this
value in combination with the value RT can be used to calculate a
forming limit curve to allow for failure. 
Sheet  thickness  used  for  calculating  a  forming  limit  curve.    This
value does not override the sheet thickness in any way.  It is only
used in conjunction with the parameter RN to calculate a forming
limit curve if the parameter FLDCID is not defined.   
FLDSAFE 
A  safety  offset  of  the  forming  limit  curve.    This  value  should  be
input as a percentage (ex.  10 not 0.10).  This safety margin will be
applied  to  the  forming  limit  curve  defined  by  FLDCID  or  the
curve calculated by RN and RT. 
FLDNIPF 
Numerical integration points failure treatment. 
GT.0.0: The number of element integration points that must fail
before    the  element  is  deleted.    By  default,  if  one  inte-
gration point has strains above the forming limit curve,
the element is flagged for deletion. 
LT.0.0:  The  element  is  deleted  when  all  integration  points 
within  a  relative  distance  of  –FLDNIPF  from  the  mid 
surface have failed (value between -1.0 and 0.0).  
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3. 
D1, D2, D3 
Components of vector 𝐝 for AOPT = 2. 
BETA 
Material angle in degrees for AOPT = 0 and 3, may be overridden 
on the element card, see *ELEMENT_SHELL_BETA.
See material 36 for the theoretical basis. 
*MAT_FLD_3-PARAMETER_BARLAT 
The forming limit curve can be input directly as a curve by specifying a load curve id 
with the parameter FLDCID.  When defining such a curve, the major and minor strains 
must be input as percentages. 
Alternatively, the parameters RN and RT can be used to calculate a forming limit curve.  
The use of RN and RT is not recommended for non-ferrous materials.  RN and RT are 
ignored if a non-zero FLDCID is defined. 
The first history variable is the maximum strain ratio defined by: 
𝜀majorworkpiece
𝜀majorfld
corresponding  to  𝜀minorworkpiece.    A  value  between  0  and  1  indicates  that  the  strains  lie 
below  the  forming  limit  curve.    Values  above  1  indicate  that  the  strains  are  above  the 
forming limit curve.
*MAT_191 
Purpose:    This  is  Material  Type  191.    This  material  enables  lumped  plasticity  to  be 
developed at the ‘node 2’ end of Belytschko-Schwer beams (resultant formulation).  The 
plastic yield surface allows interaction between the two moments and the axial force. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
F 
F 
4 
5 
6 
7 
8 
PR 
ASFLAG 
FTYPE 
DEGRAD 
IFEMA 
Default 
none 
none 
none 
none 
0.0 
  Card 2 
1 
2 
3 
4 
5 
I 
1 
6 
I 
0 
7 
I 
0 
8 
Variable 
LCPMS 
SFS 
LCPMT 
SFT 
LCAT 
SFAT 
LCAC 
SFAC 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
1.0 
LCMPS
1.0 
none 
1.0 
LCAT 
1.0 
This card 3 format is used when FTYPE = 1 (default).  
  Card 3 
1 
2 
3 
4 
Variable 
ALPHA 
BETA 
GAMMA 
DELTA 
Type 
F 
F 
F 
F 
5 
A 
F 
6 
B 
F 
7 
8 
FOFFS 
F 
Default  see note  see note  see note see note see note see note 
0.0
This card 3 format is used when FTYPE = 2. 
  Card 3 
1 
Variable 
SIGY 
Type 
F 
2 
D 
F 
3 
W 
F 
4 
TF 
F 
5 
TW 
F 
Default 
none 
none 
none 
none 
none 
6 
7 
8 
This card 3 format is used when FTYPE = 4. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PHI_T 
PHI_C 
PHI_B 
Type 
F 
F 
F 
Default 
0.8 
0.85 
0.9 
This card 3 format is used when FTYPE = 5. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ALPHA 
BETA 
GAMMA 
DELTA 
PHI_T 
PHI_C 
PHI_B 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
1.4 
none 
1.0 
1.0 
1.0
FEMA limits Card 1.  Additional card for IFEMA > 0. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PR1 
PR2 
PR3 
PR4 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
FEMA limits Card 2.  Additional card for IFEMA = 2. 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TS1 
TS2 
TS3 
TS4 
CS1 
CS2 
CS3 
CS4 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
F 
F 
F 
TS1 
TS2 
TS3 
TS4 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
ASFLAG 
Axial  strain  definition  for  force-strain  curves,  degradation  and 
FEMA output: 
EQ.0.0: true (log) total strain 
EQ.1.0: change in length 
EQ.2.0: nominal total strain 
EQ.3.0: FEMA  plastic  strain  ( = nominal  total  strain  minus 
elastic strain)
*MAT_SEISMIC_BEAM 
DESCRIPTION
FTYPE 
Formulation type for interaction 
EQ.1: Parabolic  coefficients,  axial  load  and  biaxial  bending
(default). 
EQ.2: Japanese code, axial force and major axis bending.  
EQ.4:  AISC utilization calculation but no yielding 
EQ.5:  AS4100 utilization calculation but no yielding 
DEGRADE 
Flag for degrading moment behavior  
EQ.0: Behavior as in previous versions 
EQ.1: Fatigue-type degrading moment-rotation behavior 
EQ.2: FEMA-type degrading moment-rotation behavior 
IFEMA 
Flag for input of FEMA thresholds 
EQ.0: No input 
EQ.1: Input of rotation thresholds only 
EQ.2: Input of rotation and axial strain thresholds 
LCPMS 
Load curve ID giving plastic moment vs.  Plastic rotation at node
2 about local s-axis.  See *DEFINE_CURVE. 
SFS 
Scale factor on s-moment at node 2. 
LCPMT 
Load curve ID giving plastic moment vs.  Plastic rotation at node
2 about local t-axis.  See *DEFINE_CURVE. 
SFT 
LCAT 
SFAT 
LCAC 
Scale factor on t-moment at node 2. 
Load  curve  ID  giving  axial  tensile  yield  force  vs.    total  tensile
(elastic + plastic) strain or vs.  elongation.  See AOPT above.  All 
values are positive.  See *DEFINE_CURVE. 
Scale factor on axial tensile force. 
Load  curve  ID  giving  compressive  yield  force  vs. 
  total
compressive (elastic + plastic) strain or vs.  elongation.  See AOPT
above.  All values are positive.  See *DEFINE_CURVE. 
SFAC 
Scale factor on axial tensile force. 
ALPHA 
Parameter to define yield surface.
VARIABLE   
DESCRIPTION
BETA 
Parameter to define yield surface. 
GAMMA 
Parameter to define yield surface. 
DELTA 
Parameter to define yield surface. 
A 
B 
Parameter to define yield surface. 
Parameter to define yield surface. 
FOFFS 
Force offset for yield surface . 
SIGY 
Yield stress of material. 
D 
W 
TF 
TW 
PHI_T 
PHI_C 
PHI_B 
Depth of section used to calculate interaction curve. 
Width of section used to calculate interaction curve. 
Flange thickness of section used to calculate interaction curve. 
Web thickness used to calculate interaction curve. 
Factor on tensile capacity, φt 
Factor on compression capacity, φc 
Factor on bending capacity, φb 
PR1 - PR4 
Plastic rotation thresholds 1 to 4 
TS1 - TS4 
Tensile axial strain thresholds 1 to 4 
CS1 - CS4 
Compressive axial strain thresholds 1 to 4 
Remarks: 
Yield surface for formulation type 1 is of the form: 
𝜓 = (
𝑀𝑠
𝑀𝑦𝑠
)
+ (
𝑀𝑡
𝑀𝑦𝑡
)
+ 𝐴 (
𝐹𝑦
)
+ 𝐵 (
)
− 1 
𝐹𝑦
Where, 
𝑀𝑠, 𝑀𝑡 = moments about local s and t axes 
𝑀𝑦𝑠, 𝑀𝑦𝑡 = current yield moments 
𝐹 = axial force
𝐹𝑦 = Yield force; LCAC in compression or LCAT in tension 
𝛼, 𝛽, 𝛾, 𝛿 = Input parameters; must be greater than or equal to 1.1 
𝐴, 𝐵 = input paramaters 
If  α, β, γ, δ, A and B are all set to zero then the following default values are used: 
ALPHA 
BETA   
GAMMA 
DELTA 
A 
B 
=  
 =  
 =  
=  
 =  
 =  
 2.0 
 2.0 
 2.0 
 4.0 
 2.0 
-1.0 
FOFFS offsets the yield surface parallel to the axial force axis.  It is the compressive axial 
force  at  which  the  maximum  bending  moment  capacity  about  the  local  s-axis 
(determined by LCPMS and SFS), and that about the local t-axis (determined by LCPMT 
and SFT), occur.  For steel beams and columns, the value of FOFFS is usually zero.  For 
reinforce  concrete  beams,  columns  and  shear  walls,  the  maximum  bending  moment 
capacity occurs corresponding to a certain compressive axial force, FOFFS.  The value of 
FOFFS  can  be  input  as  either  positive  or  negative.    Internally,  LS-DYNA  converts 
FOFFS to, and regards compressive axial force as, negative. 
Interaction surface FTYPE 4 calculates a utilisation parameter using the yield force and 
moment data given on card 2, but the elements remain elastic even when the forces or 
moments  exceed  yield  values.    This  is  done  for  consistency  with  the  design  code  OBE 
AISC LRFD (2000).  The utilisation calculation is as follows: 
Ultilisation =
𝐾1𝐹
𝜙𝐹𝑦
+
𝐾2
𝜙𝑏
(
𝑀𝑠
𝑀𝑦𝑠
+
𝑀𝑡
𝑀𝑦𝑡
) 
where, 
and, 
𝑀𝑠, 𝑀𝑡𝑀𝑦𝑠, 𝑀𝑦𝑡, 𝐹𝑦 are defined as in the preceding equation 
𝜙 = from PHI_ T under tension; PHI_ C under compression 
𝜙𝑏 = take from PHI_ B 
𝐾1 =
0.5
1.0
⎧
{{{
⎨
{{{
⎩
𝜙𝐹𝑦
𝜙𝐹𝑦
< 0.2
≥ 0.2
𝐾2 =
1.0
9⁄
⎧
{{{
⎨
{{{
⎩
𝜙𝐹𝑦
𝜙𝐹𝑦
< 0.2
≥ 0.2
Interaction surface FTYPE  5 is similar to type 4 (calculates a utilisation parameter using 
the yield data, but the elements do not yield).  The equations are taken from Australian 
code AS4100.  The user must select appropriate values of α, β, γ and δ using the various 
clauses of Section 8 of AS4100.  It is assumed that the local s-axis  is the major axis for 
bending. 
Utilisation = max(𝑈1, 𝑈2, 𝑈3, 𝑈4, 𝑈5) 
𝑈1 =
𝑈2 =
𝛽𝜙𝑐𝐹𝑦𝑐
𝜙𝑡𝐹𝑦𝑡
𝑈3 = [
𝑈4 = [
𝑀𝑠
𝐾2𝜙𝑏𝑀𝑦𝑠
𝑀𝑠
𝐾4𝜙𝑏𝑀𝑦𝑠
𝜙𝑐𝐹𝑦𝑐
+
]
]
+ [
+ [
𝑀𝑠
𝜙𝑏𝑀𝑦𝑠
+
𝑀𝑡
𝐾1𝜙𝑏𝑀𝑦𝑡
𝑀𝑡
𝐾3𝜙𝑏𝑀𝑦𝑡
𝑀𝑡
𝜙𝑏𝑀𝑦𝑡
used for members in compression
used for members in tension
used for members in compression
used for members in tension
used for all members
]
]
𝑈5 =
where, 
and, 
𝑀𝑠, 𝑀𝑡, 𝐹, 𝑀𝑦𝑠, 𝑀𝑦𝑡, 𝐹𝑦𝑡, 𝐹𝑦𝑐 are  as defined above 
𝐾1 = 1.0 −
𝛽𝜙𝑐𝐹𝑦𝑐
𝐾2 = min [𝐾1, 𝛼 (1.0 −
𝛿𝜙𝑐𝐹𝑦𝑐
)] 
𝐾3 = 1.0 −
𝜙𝑡𝐹𝑦𝑡
𝐾4 = min [K3, 𝛼 (1.0 +
𝜙𝑡𝐹𝑦𝑡
)] 
where 
𝐾1, 𝐾2, 𝐾3𝐾4 are subject to a minimum value of 10−6, 
𝛼, 𝛽, 𝛾, 𝛿, 𝜙𝑡, 𝜙𝑐, 𝜙𝑏 are input parameters 
The  option  for  degrading  moment  behavior  changes  the  meaning  of  the  plastic 
moment-rotation curve as follows:
If  DEGRAD = 0  (not  recommended),  the  x-axis  points  on  the  curve  represent  current 
plastic  rotation  (i.e.    total  rotation  minus  the  elastic  component  of  rotation).    This 
quantity  can  be  positive  or  negative  depending  on  the  direction  of  rotation;  during 
hysteresis the behavior will repeatedly follow backwards and forwards along the same 
curve.    The  curve  should  include  negative  and  positive  rotation  and  moment  values.  
This option is retained so that results from existing models will be unchanged. 
If  DEGRAD = 1,  the  x-axis  points  represent  cumulative  absolute  plastic  rotation.    This 
quantity  is  always  positive,  and  increases  whenever  there  is  plastic  rotation  in  either 
direction.  Thus, during hysteresis, the yield moments are taken from points in the input 
curve  with  increasingly  positive  rotation.    If  the  curve  shows  a  degrading  behavior 
(reducing  moment  with  rotation),  then,  once  degraded  by  plastic  rotation,  the  yield 
moment can never recover to its initial value.  This option can be thought of as having 
“fatigue-type”  hysteretic  damage  behavior,  where  all  plastic  cycles  contribute  to  the 
total damage. 
If DEGRAD = 2, the x-axis points represent the high-tide value (always positive) of the 
plastic rotation.  This quantity increases only when the absolute value of plastic rotation 
exceeds the previously recorded maximum.  If smaller cycles follow a larger cycle, the 
plastic  moment  during  the  small  cycles  will  be  constant,  since  the  high-tide  plastic 
rotation  is  not  altered  by  the  small  cycles.    Degrading  moment-rotation  behavior  is 
possible.    This  option  can  be  thought  of  as  showing  rotation-controlled  damage,  and 
follows the FEMA approach for treating fracturing joints. 
DEGRAD  applies  also  to  the  axial  behavior.    The  same  options  are  available  as  for 
rotation: DEGRAD = 0 gives unchanged behavior from previous versions; DEGRAD = 1 
gives  a  fatigue-type  behavior  using  cumulative  plastic  strain;  and  DEGRAD = 2  gives 
FEMA-type  behavior,  where  the  axial  load  capacity  depends  on  the  high-tide  tensile 
and compressive strains.  The definition of strain for this purpose is according to AOPT 
on  Card  1  –  it  is  expected  that  AOPT = 2  will  be  used  with  DEGRAD = 2.    The  “axial 
strain” variable plotted by post-processors is the variable defined by AOPT. 
The  output  variables  plotted  as  “plastic  rotation”  have  special  meanings  for  this 
material model as follows – note that hinges form only at Node 2: 
 “Plastic rotation at End 1” is really a high-tide mark of absolute plastic rotation at Node 
2, defined as follows: 
1.  Current  plastic  rotation  is  the  total  rotation  minus  the  elastic  component  of 
rotation. 
2.  Take the absolute value of the current plastic rotation, and record the maximum 
achieved up to the current time.  This is the high-tide mark of plastic rotation.
If DEGRAD = 0, “Plastic rotation at End 2” is the current plastic rotation at Node 2. 
If DEGRAD = 1 or 2, “Plastic rotation at End 2” is the current total rotation at Node 2. 
The  total  rotation  is  a  more  intuitively  understood  parameter,  e.g.    for  plotting 
hysteresis  loops.    However,  with  DEGRAD = 0,  the  previous  meaning  of  that  output 
variable has been retained such that results from existing models are unchanged.  
FEMA  thresholds  are  the  plastic  rotations  at  which  the  element  is  deemed  to  have 
passed  from  one  category  to  the  next,  e.g.    “Elastic”,  “Immediate  Occupancy”,  “Life 
Safe”, etc.  The high-tide plastic rotation (maximum of Y and Z) is checked against the 
user-defined limits FEMA1, FEMA2, etc.  The output flag is then set to 0, 1, 2, 3, or 4: 0 
means  that  the  rotation  is  less  than  FEMA1;  1  means  that  the  rotation  is  between 
FEMA1  and  FEMA2,  and  so  on.    By  contouring  this  flag,  it  is  possible  to  see  quickly 
which joints have passed critical thresholds.  
For this material model, special output parameters are written to the d3plot and d3thdt 
files.  The number of output parameters for beam elements is automatically increased to 
20  (in  addition  to  the  six  standard  resultants)  when  parts  of  this  material  type  are 
present.    Some  post-processors  may  interpret  this  data  as  if  the  elements  were 
integrated beams with 4 integration points.  Depending on the post-processor used, the 
data may be accessed as follows: 
Extra variable 16 (or Integration point 4 Axial Stress):  
Extra variable 17 (or Integration point 4 XY Shear Stress):   Current utilization 
Extra variable 18 (or Integration point 4 ZX Shear Stress):   Maximum  utilization 
FEMA rotation flag 
to 
Extra variable 20 (or Integration point 4 Axial Strain):  
date 
FEMA axial flag 
“Utilization” is the yield parameter, where 1.0 is on the yield surface.
*MAT_SOIL_BRICK 
Purpose:  This is Material Type 192.  It is intended for modeling over-consolidated clay. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
RO 
RLAMDA  RKAPPA 
RIOTA 
RBETA1 
RBETA2 
RMU 
Type 
A8 
F 
F 
F 
F 
F 
F 
F 
Default 
1.0 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RNU 
RLCID 
TOL 
PGCL 
SUB-INC 
BLK 
GRAV 
THEORY 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0005 
9.807 
I 
0 
Additional card for THEORY > 0. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RVHHH 
XSICRIT 
ALPHA 
RVH 
RNU21 
ANISO_4 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density 
RLAMDA 
Material coefficient
VARIABLE   
DESCRIPTION
RKAPPA 
Material coefficient 
RIOTA 
Material coefficient 
RBETA1 
Material coefficient 
RBETA2 
Material coefficient 
RMU 
Shape factor coefficient.  This parameter will modify the shape of 
the yield surface used.  1.0 implies a von Mises type surface, but
1.1 to 1.25 is more indicative of soils.  The default value is 1.0. 
RNU 
Poisson’s ratio 
RLCID 
TOL 
PGCL 
SUB-INC 
BLK 
GRAV 
Load curve identification number referring to a curve defining up
to 10 pairs of ‘string-length’ vs G/Gmax points. 
User defined tolerance for convergence checking.  Default value is
set to 0.02. 
Pre-consolidation  ground  level.    This  parameter  defines  the 
maximum surface level (relative to z = 0.0 in the model) of the soil 
throughout  geological  history. 
  This  is  used  calculate  the
maximum over burden pressure on the soil elements. 
User  defined  strain  increment  size.    This  is  the  maximum  strain
increment that the material model can normally cope with.  If the
value is exceeded a warning is echoed to the d3hsp file. 
The  elastic  bulk  stiffness  of  the  soil.    This  is  used  for  the  contact 
stiffness only. 
The  gravitational  acceleration.    This  is  used  to  calculate  the
element  stresses  due  the  overlying  soil.      Default  is  set  to  9.807
m/s2. 
THEORY 
Version of material subroutines used . 
EQ.0: 1995 version, vectorized (Default) 
EQ.4: 2003 version, unvectorized 
RVHHH 
Anisotropy ratio Gvh / Ghh (default = Isotropic behavior) 
XSICRIT 
Anisotropy parameter
*MAT_SOIL_BRICK 
DESCRIPTION
ALPHA 
Anisotropy parameter 
RVH 
Anisotropy ratio Ev / Eh 
RNU21 
Anisotropy ratio 𝜈2/𝜈1 
ANISO_4 
Anisotropy parameter 
Remarks: 
1.  This  material  type  requires  that  the  model  is  oriented  such  that  the  z-axis  is 
defined  in  the  upward  direction.    Compressive  initial  stress  must  be  defined, 
e.g.  using *INITIAL_STRESS_SOLID or *INITIAL_STRESS_DEPTH. 
The recommended unit system is kN, meters, seconds, tonnes.  There are some 
built-in defaults that assume stress units of KN/m2. 
Over-consolidated  clays  have  suffered  previous  loading  to  higher stress  levels 
than are present at the start of the analysis.  This could have occurred due to ice 
sheets during previous ice ages, or the presence of soil or rock that has subse-
quently been eroded.  The maximum vertical stress during that time is assumed 
to be: 
𝜎VMAX = RO × GRAV × (PGCL − 𝑍el) 
where 
RO, GRAV, and PGCL = input parameters 
𝑍el = z coordinate of center of element  
Since  that time,  the  material  has  been  unloaded  until  the vertical stress  equals 
the user-defined initial vertical stress.  The previous load/unload history has a 
significant effect on subsequent behavior, e.g.  the horizontal stress in an over-
consolidated clay may be greater than the vertical stress. 
This  material  model  creates  a  load/unload cycle  for  a  sample  element  of  each 
material  of  this  type,  stores  in  a  scratch  file  the  horizontal  stress  and  history 
variables  as  a  function  of  the  vertical  stress,  and  interpolates  these  quantities 
from  the  defined  initial  vertical  stress  for  each  element.    Therefore  the  initial 
horizontal stress seen in the output files will be different from the input initial 
horizontal stress. 
This material model is developed for a Geotechnical FE program (Oasys Ltd.’s 
SAFE)  written  by  Arup.    The  default  THEORY = 0  gives  a  vectorized  version 
ported from SAFE in the 1990’s.  Since then the material model has been devel-
oped  further  in  SAFE;  the  most  recent  porting  is  accessed  using  THEORY = 4
(recommended);  however,  this  version  is  not  vectorized  and  will  run  more 
slowly on most computer platforms. 
2.  The shape factor for a typical soil would be 1.25.  Do not use values higher than 
1.35.
*MAT_DRUCKER_PRAGER 
Purpose:    This  is  Material  Type  193.    This  material  enables  soil  to  be  modeled 
effectively.    The  parameters  used  to  define  the  yield  surface  are  familiar  geotechnical 
parameters (i.e.  angle of friction).  The modified Drucker-Prager yield surface is used in 
this  material  model  enabling  the  shape  of  the  surface  to  be  distorted  into  a  more 
realistic definition for soils. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
RO 
GMOD 
RNU 
RKF 
PHI 
CVAL 
PSI 
Type 
A8 
F 
F 
F 
F 
F 
F 
F 
Default 
1.0 
0.0 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
STR_LIM 
Type 
F 
Default 
0.005 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  GMODDP 
PHIDP 
CVALDP 
PSIDP 
GMODGR
PHIGR 
CVALGR 
PSIGR 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density
VARIABLE   
DESCRIPTION
GMOD 
Elastic shear modulus 
RNU 
RKF 
PHI 
Poisson’s ratio 
Failure surface shape parameter 
Angle of friction (radians) 
CVAL 
Cohesion value 
PSI 
Dilation angle (radians) 
STR_LIM 
Minimum shear strength of material is given by STR_LIM*CVAL
GMODDP 
Depth at which shear modulus (GMOD) is correct 
PHIDP 
Depth at which angle of friction (PHI) is correct 
CVALDP 
Depth at which cohesion value (CVAL) is correct 
PSIDP 
Depth at which dilation angle (PSI) is correct 
GMODGR 
Gradient at which shear modulus (GMOD) increases with depth 
PHIGR 
Gradient at which friction angle (PHI) increases with depth 
CVALGR 
Gradient at which cohesion value (CVAL) increases with depth 
PSIGR 
Gradient at which dilation angle (PSI) increases with depth 
Remarks: 
1.  This  material  type  requires  that  the  model  is  oriented  such  that  the  z-axis  is 
defined in the upward direction.  The key parameters are defined such that may 
vary with depth (i.e.  the z-axis). 
2.  The  shape  factor  for  a  typical  soil  would  be  0.8,  but  should  not  be  pushed 
further than 0.75. 
3. 
If STR_LIM is set to less than 0.005, the value is reset to 0.005. 
4.  The yield function is defined as: 
t – p.tanβ – d = 0 
where:
p = hydrostatic stress = J1/3 
t = (q/2){a – b(r/q)3} 
q = Von Mises stress = √(3J2) 
a = 1 + 1/K     
b = 1 – 1/K 
K = input parameter RKF 
r = (27 J3/2)1/3 
J2,J3 = second and third deviatoric stress invariants 
tanβ = 6 sinφ / (3-sinφ) 
d = 6 C cosφ / (3-sinφ) 
φ= input parameter PHI 
C = input parameter CVAL
*MAT_194 
Purpose:    This  is  Material  Type  194.   It  is  for  shell  elements  only.   It  uses  empirically-
derived  algorithms  to  model  the  effect  of  cyclic  shear  loading  on  reinforced  concrete 
walls.  It is primarily intended for modeling squat shear walls, but can also be used for 
slabs.    Because  the  combined  effect  of  concrete  and  reinforcement  is  included  in  the 
empirical data, crude meshes can be used.  The model has been designed such that the 
minimum amount of input is needed: generally, only the variables on the first card need 
to be defined. 
NOTE: This material does not support specification of a ma-
terial  angle,  𝛽𝑖,  for  each  through-thickness  integra-
tion point of a shell. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
6 
7 
TMAX 
F 
8 
I 
Default 
none 
none 
none 
0.0 
0.0 
Include  the  following  data  if  “Uniform  Building  Code”  formula  for  maximum  shear 
strength or tensile cracking are required – otherwise leave blank.  
  Card 2 
Variable 
1 
FC 
2 
3 
4 
5 
6 
PREF 
FYIELD 
SIG0 
UNCONV 
ALPHA 
Type 
F 
F 
F 
F 
F 
F 
7 
FT 
F 
8 
ERIENF 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0
Variable 
Type 
1 
A 
F 
*MAT_RC_SHEAR_WALL 
2 
B 
F 
3 
C 
F 
4 
D 
F 
5 
E 
F 
6 
F 
F 
7 
8 
Default 
0.05 
0.55 
0.125 
0.66 
0.25 
1.0 
  Card 4 
Variable 
1 
Y1 
Type 
F 
2 
Y2 
F 
3 
Y3 
F 
4 
Y4 
F 
5 
Y5 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 5 
Variable 
1 
T1 
Type 
F 
2 
T2 
F 
3 
T3 
F 
4 
T4 
F 
5 
T5 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
6 
7 
8 
6 
7 
8 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
AOPT 
Type 
F 
Default 
0.0
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
3 
ZP 
F 
4 
A1 
F 
5 
A2 
F 
6 
A3 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
*MAT_194 
7 
8 
  Card 8 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
7 
8 
BETA 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
TMAX 
FC 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Young’s Modulus 
Poisson’s Ratio 
Ultimate  in-plane  shear  stress.    If  set  to  zero,  LS-DYNA  will 
calculate  TMAX  based  on  the  formulae  in  the  Uniform  Building
Code, using the data on card 2.  See Remarks. 
Unconfined  Compressive  Strength  of  concrete  (used  in  the
calculation  of  ultimate  shear  stress;  crushing  behavior  is  not 
modeled) 
PREF 
Percent reinforcement, e.g.  if 1.2% reinforcement, enter 1.2 
FYIELD 
Yield stress of reinforcement 
SIG0 
Overburden  stress  (in-plane  compressive  stress)  -  used  in  the 
calculation of ultimate shear stress.  Usually sig0 is left as zero.
*MAT_RC_SHEAR_WALL 
DESCRIPTION
UCONV 
Unit conversion factor.  UCONV is expected to be set such that, 
UCONV = √1.0 PSI  in the model's stress units. 
This used to convert the ultimate tensile stress of concrete which
is  expressed  as  √FC  where  FC  is  given  in  PSI.    Therefore  a  unit 
conversion factor of √PSI Stress Unit
 is required.  Examples: 
⁄
UCONV = 83.3 = √6894 if stress unit is N/m2 
UCONV = 0.083 if stress unit is MN/m2 or N/mm2  
ALPHA 
Shear span factor - see below. 
FT 
ERIENF 
A 
B 
C 
D 
E 
F 
Cracking stress in direct tension - see notes below.  Default is 8% 
of the cylinder strength. 
Young’s  Modulus  of  reinforcement.    Used  in  calculation  of  post-
cracked stiffness - see notes below. 
Hysteresis  constants  determining  the  shape  of  the  hysteresis 
loops. 
Hysteresis  constants  determining  the  shape  of  the  hysteresis
loops. 
Hysteresis  constants  determining  the  shape  of  the  hysteresis
loops. 
Hysteresis  constants  determining  the  shape  of  the  hysteresis
loops. 
Hysteresis  constants  determining  the  shape  of  the  hysteresis 
loops. 
Strength  degradation  factor.    After  the  ultimate  shear  stress  has
been  achieved,  F  multiplies  the  maximum  shear  stress  from  the
curve  for  subsequent  reloading.    F = 1.0  implies  no  strength 
degradation (default).  F = 0.5 implies that the strength is halved 
for subsequent reloading. 
Y1, Y2, …, Y5 
Engineering shear strain points on stress-strain curve.  By default 
these  are  calculated  from  the  values  on  card  1.    See  below  for
more guidance.
VARIABLE   
T1, T2, …, T5 
DESCRIPTION
Shear  stress  points  on  stress-strain  curve.    By  default  these  are 
calculated  from  the  values  on  card  1.    See  below  for  more
guidance. 
AOPT 
Material axes option: 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element  nodes  as  shown  in  Figure  M2-1,  and  then  ro-
tated  about  the  shell  element  normal  by  the  angle  BE-
TA.  Nodes 1, 2, and 4 of an element are identical to the
nodes used for the definition of a coordinate system as
by *DEFINE_COORDINATE_NODES. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: applicable  to  shell  elements  only. 
  This  option
determines  locally  orthotropic  material  axes  by  offset-
ting the material axes by an angle to be specified from
a line in the plane of the shell determined by taking the
cross  product  of  the  vector  v  defined  below  with  the
shell normal vector. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID 
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
XP, YP, ZP 
Coordinates of point 𝐩 for AOPT = 1. 
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3. 
D1, D2, D3 
Components of vector 𝐝 for AOPT = 2. 
BETA 
Material angle in degrees for AOPT = 0 and 3, may be overridden 
on the element card, see *ELEMENT_SHELL_BETA. 
Remarks: 
The  element  is  linear  elastic  except  for  in-plane  shear  and  tensile  cracking  effects.  
Crushing due to direct compressive stresses are modeled only insofar as there is an in-
plane  shear  stress  component.    It  is  not  recommended  that  this  model  be  used  where 
nonlinear response to direct compressive or loads is important. 
Note that the in-plane shear stress 𝑡𝑥𝑦 is defined as the shear stress in the element’s local 
𝑥-𝑦  plane.    This  is  not  necessarily  equal  to the  maximum  shear  stress  in  the  plane:  for 
example,  if  the  principal  stresses  are  at  45  degrees  to  the  local  axes,  𝑡𝑥𝑦  is  zero.  
Therefore it is important to ensure that the local axes are appropriate - for a shear wall 
the local axes should be vertical or horizontal.  By default, local 𝑥 points from node 1 to 
node 2 of the element.  It is possible to change the local axes by using AOPT > 0. 
If  TMAX  is  set  to  zero,  the  ultimate  shear  stress  is  calculated  using  a  formula  in  the 
Uniform Building Code 1997, section 1921.6.5: 
TMAXUBC = UCONV × ALPHA × √FC + RO × FY 
where, 
UCONV = unit conversion factor, see varriable list
ALPHA = aspect ratio
= 2.0 for  ℎ 𝑙⁄ ∈ (2.0, ∞) increases linearly to 3.0 for  ℎ 𝑙⁄ ∈ (2.0,1.5) 
FC = unconfined compressive strength of concrete
RO = fraction of reinforcement
= (percent reinforcement) 100
⁄
FY = yield stress of reinforcement
To this we add shear stress due to the overburden to obtain the ultimate shear stress: 
TMAXUBC = TMAXUBC + SIG0 
where 
SIG0 = in plane compressive stress under static equilibrium conditions 
The  UBC  formula  for  ultimate  shear  stress  is  generally  conservative  (predicts  that  the 
wall  is  weaker  than  shown  in  test),  sometimes  by  50%  or  more.    A  less  conservative 
formula is that of Fukuzawa: 
TMAX = max [(0.4 +
𝐴𝑐
𝐴𝑤
) , 1] × 2.7 × (1.9 +
𝐿𝑣
) × UCONV+√FC + 0.5
× RO × FY + SIG0 
where 
𝐴𝐶 = Cross-sectional area of stiffening features such as columns or flanges 
𝐴𝑤 = Cross-sectional area of wall 
⁄
𝑀 𝐿𝑣⁄ = Aspect ratio of wall  height length
Other terms  are  as  above.   This  formula  is  not  included  in  the  material  model:  TMAX 
should  be  calculated  by  hand  and  entered  on  Card  1  if  the  Fukuzawa  formula  is 
required. 
It should be noted that none of the available formulae, including Fukuzawa, predict the 
ultimate  shear  stress  accurately  for  all  situations.    Variance  from  the  experimental 
results can be as great as 50%. 
The shear stress vs shear strain curve is then constructed automatically as follows, using 
the algorithm of Fukuzawa extended by Arup: 
1.  Assume ultimate engineering shear strain, 𝛾𝑢 = 0.0048 
2.  First point on curve, corresponding to concrete cracking, is at 
(0.3 ×
TMAX
, 0.3 × TMAX), 
where 𝐺 is the elastic shear modulus given by 
𝐺 =
2(1 + 𝜈)
. 
3.  Second point, corresponding to the reinforcement yield, is at 
4.  Third point, corresponding to the ultimate strength, is at 
(0.5 × 𝛾𝑢, 0.8 × TMAX). 
(𝛾𝑢, TMAX). 
5.  Fourth point, corresponding to the onset of strength reduction, is at 
6.  Fifth point, corresponding to failure is at 
(2𝛾𝑢,TMAX). 
(3𝛾𝑢, 0.6 × TMAX). 
After failure, the shear stress drops to zero.  The curve points can be entered by the user 
if desired, in which case they over-ride the automatically calculated curve.  However, it 
is anticipated that in most cases the default curve will be preferred due to ease of input. 
Hysteresis follows the algorithm of Shiga as for the squat shear wall spring .  The hysteresis constants which are defined in fields 
A, B, C, D, and E can be entered by the user if desired, but it is generally recommended 
that the default values be used. 
Cracking in tension is checked for the local x and y directions only – this is calculated 
separately from the in-plane shear.  A trilinear response is assumed, with turning points 
at concrete cracking and reinforcement yielding.  The three regimes are:
1.  Pre-cracking,  linear  elastic  response  is  assumed  using  the  overall  Young’s 
Modulus on Card 1. 
2.  Cracking  occurs  in  the  local  x  or  y  directions  when  the  tensile  stress  in  that 
direction exceeds the concrete tensile strength FT (if not input on Card 2, this 
defaults  to  8%  of  the  compressive  strength FC).    Post-cracking,  a  linear  stress-
strain  response  is  assumed  up  to  reinforcement  yield  at  a  strain  defined  by 
reinforcement yield stress divided by reinforcement Young’s Modulus. 
3.  Post-yield, a constant stress is assumed (no work hardening). 
Unloading returns to the origin of the stress-strain curve.  
For  compressive  strains  the  response  is  always  linear  elastic  using  the  overall 
Young’s Modulus on Card 1. 
If insufficient data is entered, no cracking occurs in the model.  As a minimum, 
FC and FY are needed. 
Extra variables are available for post-processing as follows: 
Extra variable 1: Current engineering shear strain 
Extra variable 2: Shear status:  0, 1, 2, 3, 4, or 5– see below 
Extra variable 3: Maximum direct strain so far in local 𝑥 direction (for ten-
sile cracking) 
Extra variable 4: Maximum direct strain so far in local 𝑦 direction (for ten-
sile cracking)  
Extra variable 5: Tensile  status:  0,  1  or  2 = elastic,  cracked,  or  yielded  re-
spectively. 
The shear status shows how far along the shear stress-strain curve each element 
has  progressed,  e.g.    status  2  means  that  the  element  has  passed  the  second 
point  on  the  curve.    These  status  levels  correspond  to  performance  criteria  in 
building design codes such as FEMA.
*MAT_195 
This  is  Material  Type  195  for  beam  elements.    An  elasto-plastic  material  with  an 
arbitrary stress versus strain curve and arbitrary strain rate dependency can be defined.  
See also Remark below.  Also, failure based on a plastic strain or a minimum time step 
size can be defined. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
6 
7 
8 
SIGY 
ETAN 
FAIL 
TDEL 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
0.0 
10.E+20  10.E+20
  Card 2 
Variable 
Type 
Default 
1 
C 
F 
0 
  Card 3 
1 
2 
P 
F 
0 
2 
3 
4 
5 
6 
7 
8 
LCSS 
LCSR 
F 
0 
3 
F 
0 
4 
5 
6 
7 
8 
Variable 
NOTEN 
TENCUT 
SDR 
Type 
Default 
I 
0 
F 
F 
E15.0 
0.0 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density.
E 
PR 
SIGY 
ETAN 
FAIL 
*MAT_CONCRETE_BEAM 
DESCRIPTION
Young’s modulus. 
Poisson’s ratio. 
Yield stress. 
Tangent modulus, ignored if (LCSS.GT.0) is defined. 
Failure flag. 
LT.0.0:  user  defined  failure  subroutine  is  called  to  determine
failure 
EQ.0.0: failure is not considered.  This option is recommended
if failure is not of interest since many calculations will
be saved. 
GT.0.0:  plastic strain to failure.  When the plastic strain reaches
this value, the element is deleted from the calculation. 
TDEL 
Minimum time step size for automatic element deletion. 
C 
P 
LCSS 
Strain rate parameter, C, see formula below. 
Strain rate parameter, P, see formula below. 
Load  curve  ID  or  Table  ID.    Load  curve  ID  defining  effective
stress  versus  effective  plastic  strain.    If  defined  EPS1-EPS8  and 
ES1-ES8  are  ignored.      The  table  ID  defines  for  each  strain  rate
value  a  load  curve  ID  giving  the  stress  versus  effective  plastic
strain for that rate, See Figure M16-1 stress versus effective plastic 
strain curve for the lowest value of strain rate is used if the strain
rate  falls  below  the  minimum  value.    Likewise,  the  stress  versus 
effective plastic strain curve for the highest value of strain rate is
used  if  the  strain  rate  exceeds  the  maximum  value.    The  strain
rate parameters: C and P; 
LCSR 
Load curve ID defining strain rate scaling effect on yield stress. 
NOTEN 
No-tension flag, 
EQ.0: beam takes tension, 
EQ.1: beam takes no tension, 
EQ.2: beam takes tension up to value given by TENCUT. 
TENCUT 
Tension cutoff value.
VARIABLE   
DESCRIPTION
SDR 
Stiffness degradation factor. 
Remarks: 
The  stress  strain  behavior  may  be  treated  by  a  bilinear  stress  strain  curve  by  defining 
the  tangent  modulus,  ETAN.    An  effective  stress  versus  effective  plastic  strain  curve 
(LCSS) may be input instead of defining ETAN.  The cost is roughly the same for either 
approach.    The  most  general  approach  is  to  use  the  table  definition  (LCSS)  discussed 
below. 
Three options to account for strain rate effects are possible. 
1.  Strain rate may be accounted for using the Cowper and Symonds model which 
scales the yield stress with the factor 
1 + (
𝑝⁄
)
𝜀̇
where 𝜀̇ is the strain rate.  𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗. 
2.  For  complete  generality  a  load  curve  (LCSR)  to  scale  the  yield  stress  may  be 
input instead.  In this curve the scale factor versus strain rate is defined. 
3. 
If different stress versus strain curves can be provided for various strain rates, 
the option using the reference to a table (LCSS) can be used.
*MAT_GENERAL_SPRING_DISCRETE_BEAM 
This  is  Material  Type  196.    This  model  permits  elastic  and  elastoplastic  springs  with 
damping to be represented with a discrete beam element of type 6 by using six springs 
each acting about one  of the six local degrees-of-freedom.  For elastic behavior, a load 
curve defines force or moment versus displacement or rotation.  For inelastic behavior, 
a load curve defines yield force or moment versus plastic deflection or rotation, which 
can vary in tension and compression. 
The two nodes defining a beam may be coincident to give a zero length beam, or offset 
to give a finite length beam.  For finite length discrete beams the absolute value of the 
variable  SCOOR  in  the  SECTION_BEAM  input  should  be  set  to  a  value  of  2.0,  which 
causes the local r-axis to be aligned along the two nodes of the beam to give physically 
correct  behavior.    The  distance  between  the  nodes  of  a  beam  should  not  affect  the 
behavior of this material model.  A triad is used to orient the beam for the directional 
springs.  
3 
4 
5 
6 
7 
8 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
Degree of Freedom Card Pairs.  For each active degree of freedom include a pair of 
cards 2 and 3.   This data is terminated by the next keyword (“*”) card or when all six 
degrees of freedom have been specified. 
  Card 2 
1 
2 
Variable 
DOF 
TYPE 
Type 
I 
  Card 3 
1 
I 
2 
Variable 
FLCID 
HLCID 
Type 
F 
F 
3 
K 
F 
3 
C1 
F 
4 
D 
F 
4 
C2 
F 
5 
6 
7 
8 
CDF 
TDF 
F 
5 
F 
6 
DLE 
GLCID 
F 
I 
7
VARIABLE   
DESCRIPTION
MID 
RO 
DOF 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density, see also volume in *SECTION_BEAM definition. 
Active  degree-of-freedom,  a  number  between  1  and  6  inclusive.
Each value of DOF can only be used once.  The active degree-of-
freedom  is  measured  in  the  local  coordinate  system  for  the
discrete beam element. 
TYPE 
The default behavior is elastic.  For inelastic behavior input 1. 
K 
D 
CDF 
TDF 
FLCID 
Elastic  loading/unloading  stiffness.    This  is  required  input  for
inelastic behavior. 
Optional viscous damping coefficient. 
Compressive displacement at failure.  Input as a positive number.
After failure, no forces are carried.  This option does not apply to
zero length springs. 
EQ.0.0:  inactive. 
Tensile  displacement  at  failure.    After  failure,  no  forces  are
carried. 
EQ.0.0:  inactive. 
Load curve ID, see *DEFINE_CURVE.  For option TYPE = 0, this 
curve  defines  force  or  moment  versus  deflection  for  nonlinear
elastic behavior.  For option TYPE = 1, this curve defines the yield 
force versus plastic deflection.  If the abscissa of the first point of 
the  curve  is  0.    the  force  magnitude  is  identical  in  tension  and
compression, i.e., only the sign changes.  If not, the yield stress in
the  compression  is  used  when  the  spring  force  is  negative.    The
plastic displacement increases monotonically in this implementa-
tion.  The load curve is required input. 
HLCID 
Load  curve  ID,  see  *DEFINE_CURVE,  defining  force  versus 
relative velocity (Optional).  If the origin of the curve is at (0,0) the
force magnitude is identical for a given magnitude of the relative 
velocity, i.e., only the sign changes. 
C1 
C2 
Damping coefficient. 
Damping coefficient
*MAT_GENERAL_SPRING_DISCRETE_BEAM 
DESCRIPTION
DLE 
Factor to scale time units. 
GLCID 
Optional  load  curve  ID,  see  *DEFINE_CURVE,  defining  a  scale 
factor versus deflection for load curve ID, HLCID.  If zero, a scale
factor of unity is assumed. 
Remarks: 
If  TYPE = 0,  elastic  behavior  is  obtained.    In  this  case,  if  the  linear  spring  stiffness  is 
used, the force, F, is given by: 
𝐹 = K × Δ𝐿 + D × Δ𝐿̇ 
but if the load curve ID is specified, the force is then given by: 
𝐹 = 𝐾 𝑓 (Δ𝐿) [1 + C1 × Δ𝐿̇ + C2 × sgn(Δ𝐿̇)ln (max {1. ,
∣Δ𝐿̇∣
DLE
})] + D×Δ𝐿̇ + 𝑔(Δ𝐿)ℎ(Δ𝐿̇) 
In these equations, Δ𝐿 is the change in length  
Δ𝐿 = current length − initial length 
For the first three degrees of freedom the parameters on cards 2 and 3 have dimensions 
as  shown  below.    Being  angular  in  nature,  the  next  three  degrees  of  freedom  involve 
moment instead of force and angle instead of length, but are otherwise identical. 
[K] =
[D] =
⎧ [force]
{
[length]
⎨
{
⎩
unitless
[force]
[velocity]
FLCID = 0
FLCID > 0
[force][time]
[length]
=
[FLCID] = [GLCID] = ([length], [force]) 
[HLCID] = ([velocity], [force]) 
[C1] =
[time]
[length]
[C2] = unitless 
[DLE] =
[length]
[time]
If TYPE = 1, inelastic behavior is obtained.  In this case, the yield force is taken from the 
load curve: 
𝐹𝑌 = 𝐹𝑦(Δ𝐿plastic) 
where 𝐿plastic is the plastic deflection.  A trial force is computed as: 
and is checked against the yield force to determine 𝐹: 
𝐹𝑇 = 𝐹𝑛 + K × Δ𝐿̇(Δ𝑡) 
𝐹 = {𝐹𝑌
𝐹𝑇
if  𝐹𝑇 > 𝐹𝑌
if  𝐹𝑇 ≤ 𝐹𝑌 
The final force, which includes rate effects and damping, is given by: 
𝐹𝑛+1 = 𝐹 × [1 + C1 × Δ𝐿̇ + C2 × sgn(Δ𝐿̇)ln (max {1. ,
∣Δ𝐿̇∣
DLE
})] + D × Δ𝐿̇ + 𝑔(Δ𝐿)ℎ(Δ𝐿̇) 
Unless the origin of the curve starts at (0,0), the negative part of the curve is used when 
the  spring  force  is  negative  where  the  negative  of  the  plastic  displacement  is  used  to 
interpolate, 𝐹𝑦.  The positive part of the curve is used whenever the force is positive.  
The  cross  sectional  area  is  defined  on  the  section  card  for  the  discrete  beam  elements, 
See  *SECTION_BEAM.    The  square  root  of  this  area  is  used  as  the  contact  thickness 
offset if these elements are included in the contact treatment.
*MAT_SEISMIC_ISOLATOR 
This  is  Material  Type  197  for  discrete  beam  elements.    Sliding  (pendulum)  and 
elastomeric seismic isolation bearings can be modeled, applying bi-directional coupled 
plasticity theory.  The hysteretic behavior was proposed by Wen [1976] and Park, Wen, 
and  Ang  [1986].    The  sliding  bearing  behavior  is  recommended  by  Zayas,  Low  and 
Mahin  [1990].    The  algorithm  used  for  implementation  was  presented  by  Nagarajaiah, 
Reinhorn,  and  Constantinou  [1991].    Further  options  for  tension-carrying  friction 
bearings  are  as  recommended  by  Roussis  and  Constantinou  [2006]. 
  Element 
formulation  type  6  must  be  used.    Local  axes  are  defined  on  *SECTION_BEAM;  the 
default is the global axis system.  It is expected that the local z-axis will be vertical.  On 
*SECTION_BEAM SCOOR must be set to zero when using this material model. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
A 
F 
4 
5 
6 
7 
8 
BETA 
GAMMA 
DISPY 
STIFFV 
ITYPE 
F 
F 
F 
F 
I 
Default 
none 
none 
1.0 
0.5 
0.5 
0.0 
0.0 
0.0 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  PRELOAD 
DAMP 
MX1 
MX2 
MY1 
MY2 
Type 
Default 
F 
0 
F 
1.0 
F 
0 
F 
0 
F 
0 
F
Sliding Isolator Card.  This card is used for ITYPE = 0 or 2.  Leave this card blank for 
elastomeric isolator (TYPE = 1). 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FMAX 
DELF 
AFRIC 
RADX 
RADY 
RADB 
STIFFL 
STIFFTS 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
F 
F 
F 
1.0e20  1.0e20  1.0e20  STIFFV 
F 
0 
Card 4 for ITYPE = 1 or 2.   leave blank for sliding isolator ITYPE = 0:  
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FORCEY 
ALPHA 
STIFFT 
DFAIL 
FMAXYC 
FMAXXT 
FMAXYT 
YLOCK 
Type 
Default 
F 
0 
F 
0 
F 
F 
F 
F 
F 
F 
0.5 × 
STIFFV
1.0e20 
FMAX 
FMAX 
FMAX 
0.0 
  VARIABLE   
DESCRIPTION
MID 
RO 
A 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Nondimensional variable - see below 
GAMMA 
Nondimensional variable - see below 
BETA 
DISPY 
Nondimensional variable - see below 
Yield displacement (length units - must be > 0.0) 
STIFFV 
Vertical stiffness (force/length units)
ITYPE 
Type: 
*MAT_SEISMIC_ISOLATOR 
DESCRIPTION
EQ.0:  sliding (spherical or cylindrical) 
EQ.1:  elastomeric 
EQ.2:  sliding (two perpendicular curved beams) 
PRELOAD 
Vertical preload not explicitly modeled (force units) 
DAMP 
Damping ratio (nondimensional) 
MX1, MX2 
Moment factor at ends 1 and 2 in local X-direction 
MY1, MY2 
Moment factor at ends 1 and 2 in local Y-direction 
FMAX 
Maximum friction coefficient (dynamic) 
DELF 
Difference  between  maximum 
coefficient 
friction  and  static 
friction
AFRIC 
Velocity multiplier in sliding friction equation (time/length units)
RADX 
RADY 
RADB 
Radius for sliding in local X direction 
Radius for sliding in local Y direction 
Radius of retaining ring 
STIFFL 
Stiffness for lateral contact against the retaining ring 
STIFFTS 
Stiffness for tensile vertical response (sliding isolator - default = 0)
FORCEY 
ALPHA 
STIFFT 
DFAIL 
Yield force.  Used for elastomeric type (ITYPE = 1).  Leave blank 
for sliding type (0, and 2). 
Ratio  of  postyielding  stiffness  to  preyielding  stiffness.    Used  for
elastomeric type (ITYPE = 1).  Leave blank for sliding type (0, and 
2). 
Stiffness for tensile vertical response (elastomeric isolator).  Used
for elastomeric type (ITYPE = 1).  Leave blank for sliding type (0, 
and 2). 
Lateral  displacement  at  which  the  isolator  fails.    Used  for
elastomeric type (ITYPE = 1).  Leave blank for sliding type (0, and 
2).
DESCRIPTION
Max friction coefficient (dynamic)  for local Y-axis (compression). 
Used for ITYPE = 2.  Leave blank for ITYPE = 0 or 1. 
Max friction coefficient (dynamic) for local X-axis (tension).  Used 
for ITYPE = 2.  Leave blank for ITYPE = 0 or 1. 
Max friction coefficient (dynamic) for local Y-axis (tension).  Used 
for ITYPE = 2.  Leave blank for ITYPE = 0 or 1. 
Stiffness  locking  the  local  Y-displacement  (optional  -single-axis 
sliding).  Used for ITYPE = 2.  Leave blank for ITYPE = 0 or 1. 
  VARIABLE   
FMAXYC 
FMAXXT 
FMAXYT 
YLOCK 
Remarks: 
The  horizontal  behavior  of  both  types  is  governed  by  plastic  history  variables  Zx,  Zy 
that evolve according to equations given in the reference; A, gamma and beta and the 
yield displacement are the input parameters for this.  The intention is to provide smooth 
build-up,  rotation  and  reversal  of  forces  in  response  to  bidirectional  displacement 
histories  in  the  horizontal  plane.    The  theoretical  model  has  been  correlated  to 
experiments on seismic isolators. 
The RADX, RADY inputs for the sliding isolator are optional.  If left blank, the sliding 
surface is assumed to be flat.  A cylindrical surface is obtained by defining either RADX 
or  RADY;  a  spherical  surface  can  be  defined  by  setting  RADX = RADY.    The  effect  of 
the  curved  surface  is  to  add  a  restoring  force  proportional  to  the  horizontal 
displacement from the center.  As seen in elevation, the top of the isolator will follow a 
curved trajectory, lifting as it displaces away from the center. 
The  vertical  behavior  for  all  types  is  linear  elastic,  but  with  different  stiffnesses  for 
tension and compression.  By default, the tensile stiffness is zero for the sliding types. 
The vertical behavior for the elastomeric type is linear elastic; in the case of uplift, the 
tensile  stiffness  will  be  different  to  the  compressive  stiffness.    For  the  sliding  type, 
compression is treated as linear elastic but no tension can be carried. 
Vertical preload can be modeled either explicitly (for example, by defining gravity), or 
by using the PRELOAD input.  PRELOAD does not lead to any application of vertical 
force to the model.  It is added to the compression in the element before calculating the 
friction force and tensile/compressive vertical behavior. 
ITYPE = 0  is  used  to  model  a  single  (spherical)  pendulum  bearing.    Triple  pendulum 
bearings can be modelled using three of these elements in series, following the method 
described by Fenz and Constantinou 2008.  The input properties for the three elements
(given  by⎯Reff1,⎯μ1,⎯d1,  ⎯a1,  etc)  are  calculated  from  the  properties  of  the  actual  triple 
bearing (given by Reff1, μ1, d1,  a1, etc) as follows: 
ITYPE = 2  is  intended  to  model  uplift-prevention  sliding  isolators  that  consist  of  two 
perpendicular curved beams joined by a connector that can slide in slots on both beams.  
The beams are aligned in the local X and Y axes respectively.  The vertical displacement 
is  the  sum  of  the  displacements  induced  by  the  respective  curvatures  and  slider 
displacements along the two beams.  Single-axis sliding is obtained by using YLOCK to 
lock the local-Y displacement.  To resist uplift, STIFFTS must be defined (recommended 
value: same as STIFFV).  This isolator type allows different friction coefficients on each 
beam,  and  different  values  in  tension  and  compression.    The  total  friction,  taking  into 
account  sliding  velocity  and  the  friction  history  functions,  is  first  calculated  using 
FMAX and then scaled by FMAXXT/FMAX etc as appropriate.  For this reason, FMAX 
should not be zero. 
DAMP is the fraction of critical damping for free vertical vibration of the isolator, based 
on  the  mass  of  the  isolator  (including  any  attached  lumped  masses)  and  its  vertical 
stiffness.    The  viscosity  is  reduced  automatically  if  it  would  otherwise  infringe 
numerical  stability.    Damping  is  generally  recommended:  oscillations  in  the  vertical 
force would have a direct effect on friction forces in sliding isolators; for isolators with 
curved surfaces, vertical oscillations can be excited as the isolator slides up and down 
the  curved  surface.    It  may  occasionally  be  necessary  to  increase  DAMP  if  these 
oscillations become significant. 
This element has no rotational stiffness - a pin joint is assumed.  However, if required, 
moments  can  be  generated  according  to  the  vertical  load  multiplied  by  the  lateral 
displacement of the isolator.  The moment about the local X-axis (i.e.  the moment that is 
dependent on lateral displacement in the local Y-direction) is reacted on nodes 1 and 2 
of the element in the proportions MX1 and MX2 respectively.  Similarly, moments about 
the  local  Y-axis  are  reacted  in  the  proportions  MY1,  MY2.    These  inputs  effectively 
determine the location of the pin joint. 
For  example,  a  pin  at  the  base  of  the  column  could  be  modeled  by  setting 
MX1 = MY1 = 1.0,  MX2 = MY2 = 0.0  and  ensuring  that  node  1  is  on  the  foundation, 
node 2 at the base of the column - then all the moment is transferred to the foundation.  
For the same model, MX1 = MY1 = 0.0, MX2 = MY2 = 1.0 would imply a pin at the top 
of the foundation - all the moment is transferred to the column.  Some isolator designs 
have the pin at the bottom for moments about one horizontal axis, and at the top for the 
other  axis  -  these  can be  modeled  by  setting  MX1 = MY2 = 1.0,  MX2 = MY1 = 0.0.   It  is 
expected that all MX1,2, etc lie between 0 and 1, and that MX1+MX2 = 1.0 (or both can 
be  zero)  -  e.g.    MX1 = MX2 = 0.5  is  permitted  -  but  no  error  checks  are  performed  to 
ensure this; similarly for MY1 + MY2.
Density should be set to a reasonable value, say 2000 to 8000 kg/m3.  The element mass 
will be calculated as density x volume (volume is entered on *SECTION_BEAM). 
Note on values for *SECTION_BEAM: 
1.  Set ELFORM to 6 (discrete beam) 
2.  VOL (the element volume) might typically be set to 0.1m3 
3. 
INER needs to be non-zero (say 1.0) but the value has no effect on the solution 
since the element has no rotational stiffness. 
4.  CID can be left blank if the isolator is aligned in the global coordinate system, 
otherwise a coordinate system should be referenced. 
5.  By default, the isolator will be assumed to rotate with the average rotation of its 
two nodes.  If the base of the column rotates slightly the isolator will no longer 
be  perfectly  horizontal:  this  can  cause  unexpected  vertical  displacements  cou-
pled with the horizontal motion.  To avoid this, rotation of the local axes of the 
isolator can be eliminated by setting RRCON, SRCON and TRCON to 1.0.  This 
does  not  introduce  any  rotational  restraint  to  the  model,  it  only  prevents  the 
orientation of the isolator from changing as the model deforms. 
6.  SCOOR must be set to zero. 
7.  All other parameters on *SECTION_BEAM can be left blank. 
Post-processing note: as with other discrete beam material models, the force described 
in  post-processors  as  “Axial”  is  really  the  force  in  the  local  X-direction;  “Y-Shear”  is 
really the force in the local Y-direction; and “Z-Shear” is really the force in the local Z-
direction.
*MAT_JOINTED_ROCK 
This is Material Type 198.  Joints (planes of weakness) are assumed to exist throughout 
the  material  at  a  spacing  small  enough  to  be  considered  ubiquitous.    The  planes  are 
assumed to lie at constant orientations defined on this material card.  Up to three planes 
can  be  defined  for  each  material.    See  *MAT_MOHR_COULOMB  (*MAT_173)  for  a 
preferred alternative to this material model. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
RO 
GMOD 
RNU 
RKF 
PHI 
CVAL 
PSI 
Type 
A8 
F 
F 
F 
F 
F 
F 
F 
Default 
1.0 
0.0 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
STR_LIM  NPLANES  ELASTIC 
LCCPDR 
LCCPT 
LCCJDR 
LCCJT 
LCSFAC 
Type 
F 
Default 
0.005 
  Card 3 
1 
I 
0 
2 
I 
0 
3 
I 
0 
4 
I 
0 
5 
I 
0 
6 
I 
0 
7 
I 
0 
8 
Variable  GMODDP 
PHIDP 
CVALDP 
PSIDP 
GMODGR
PHIGR 
CVALGR 
PSIGR 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0
Repeat Card 4 for each plane (maximum 3 planes):  
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DIP 
STRIKE 
CPLANE  FRPLANE
TPLANE  SHRMAX 
LOCAL 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
1.e20 
0.0 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density 
GMOD 
Elastic shear modulus 
RNU 
RKF 
PHI 
Poisson’s ratio 
Failure surface shape parameter 
Angle of friction (radians) 
CVAL 
Cohesion value 
PSI 
Dilation angle (radians) 
STR_LIM 
Minimum shear strength of material is given by STR_LIM*CVAL
NPLANES 
Number of joint planes (maximum 3) 
ELASTIC 
Flag = 1 for elastic behavior only 
LCCPDR 
Load  curve  for  extra  cohesion  for  parent  material  (dynamic
relaxation) 
LCCPT 
Load curve for extra cohesion for parent material (transient) 
LCCJDR 
Load curve for extra cohesion for joints (dynamic relaxation) 
LCCJT 
Load curve for extra cohesion for joints (transient) 
LCSFAC 
Load curve giving factor on strength vs time
*MAT_JOINTED_ROCK 
DESCRIPTION
GMODDP 
Depth at which shear modulus (GMOD) is correct 
PHIDP 
Depth at which angle of friction (PHI) is correct 
CVALDP 
Depth at which cohesion value (CVAL) is correct 
PSIDP 
Depth at which dilation angle (PSI) is correct 
GMODGR 
Gradient at which shear modulus (GMOD) increases with depth 
PHIGR 
Gradient at which friction angle (PHI) increases with depth 
CVALGR 
Gradient at which cohesion value (CVAL) increases with depth 
PSIGR 
Gradient at which dilation angle (PSI) increases with depth 
DIP 
Angle of the plane in degrees below the horizontal 
DIPANG 
Plan view angle (degrees) of downhill vector drawn on the plane 
CPLANE 
Cohesion for shear behavior on plane 
PHPLANE 
Friction angle for shear behavior on plane (degrees) 
TPLANE 
Tensile strength across plane (generally zero or very small) 
SHRMAX 
Max  shear  stress  on  plane  (upper 
compression) 
limit, 
independent  of
LOCAL 
EQ.0: DIP and DIPANG are with respect to the global axes 
Remarks: 
1.  The  joint  plane  orientations  are  defined  by  the  angle  of  a  “downhill  vector” 
drawn  on  the  plane,  i.e.    the  vector  is  oriented  within  the  plane  to  obtain  the 
maximum possible downhill angle.  DIP is the angle of this line below the hori-
zontal.  DIPANG is the plan-view angle of the line (pointing down hill) meas-
ured clockwise from the global Y-axis about the global Z-axis. 
2.  The joint planes rotate with the rigid body motion of the elements, irrespective 
of whether their initial definitions are in the global or local axis system. 
3.  The full facilities of the modified Drucker Prager model for the matrix material 
can be used –  see description of Material type 193.  Alternatively, to speed up 
the calculation, the ELASTIC flag can be set to 1, in which case the yield surface
will not be considered and only RO, GMOD, RNU, GMODDP, GMODGR and 
the joint planes will be used. 
4.  This  material  type  requires  that  the  model  is  oriented  such  that  the  z-axis  is 
defined in the upward direction.  The key parameters are defined such that may 
vary with depth (i.e.  the z-axis) 
5.  The  shape  factor  for  a  typical  soil  would  be  0.8,  but  should  not  be  pushed 
further than 0.75. 
6. 
If STR_LIM is set to less than 0.005, the value is reset to 0.005. 
7.  A correction has been introduced into the Drucker Prager model, such that the 
yield surface never infringes the Mohr-Coulomb criterion.  This means that the 
model does not give the same results as a “pure” Drucker Prager model. 
8.  The  load  curves  LCCPDR,  LCCPT,  LCCJDR,  LCCJT  allow  additional  cohesion 
to be specified as a function of time.  The cohesion is additional to that specified 
in the material parameters.  This is intended for use during the initial stages of 
an  analysis  to  allow  application  of  gravity  or  other  loads  without  cracking  or 
yielding, and for the cracking or yielding then to be introduced in a controlled 
manner.    This  is  done  by  specifying  extra  cohesion  that  exceeds  the  expected 
stresses  initially,  then  declining  to  zero.    If  no  curves  are  specified,  no  extra 
cohesion is applied. 
9.  The  load  curve  for  factor  on  strength  applies  simultaneously  to  the  cohesion 
and tan (friction angle) of parent material and all joints.  This feature is intend-
ed  for  reducing  the  strength  of  the  material  gradually,  to  explore  factors  of 
safety.  If no curve is present, a constant factor of 1 is assumed.   Values much 
greater than 1.0 may cause problems with stability. 
10.  Extra  variables  for  plotting.    By  setting  NEIPH  on  *DATABASE_EXTENT_BI-
NARY to 15, the following variables can be plotted in D3PLOT and T/HIS: 
Extra Variable 1:  mobilized strength fraction for base material 
Extra Variable 2: 
Extra Variable 3: 
Extra Variable 4: 
Extra Variable 5: 
Extra Variable 6: 
Extra Variable 7: 
Extra Variable 8: 
Extra Variable 9: 
Extra Variable 10:  current shear utilization for plane 1 
Extra Variable 11:  current shear utilization for plane 2 
Extra Variable 12:  current shear utilization for plane 3 
rk0 for base material 
rlamda for base material 
 crack opening strain for plane 1 
crack opening strain for plane 2 
crack opening strain for plane 3 
crack accumulated engineering shear strain for plane 1 
crack accumulated engineering shear strain for plane 2 
crack accumulated engineering shear strain for plane 3
Extra Variable 13:  maximum shear utilization to date for plane 1 
Extra Variable 14:  maximum shear utilization to date for plane 2 
Extra Variable 15:  maximum shear utilization to date for plane 3 
11.  Joint  planes  would  generally  be  defined  in  the  global  axis  system  if  they  are 
taken from survey data.  However, the material model can also be used to rep-
resent  masonry,  in  which  case  the  weak  planes  represent  the  cement  and  lie 
parallel to the local element axes.
*MAT_HYSTERETIC_REINFORCEMENT 
This  is  Material  Type  203  in  LS-DYNA.    It is  intended  as  an  alternative  reinforcement 
model for layered reinforced concrete shell elements, for use in seismic analysis where 
the  nonlinear  hysteretic  behaviour  of  the  reinforcement  is  important.    *PART_COM-
POSITE or *INTEGRATION_BEAM should be used to define some integration points as 
a  part  made  of  *MAT_HYSTERETIC_REINFORCEMENT,  while  other  integration 
points  have  concrete  properties  using  *MAT_CONCRETE_EC2.    When  using  beam 
elements, ELFORM = 1 is required. 
  Card 1 
1 
Variable 
MID 
Type 
I 
2 
RO 
F 
3 
YM 
F 
4 
PR 
F 
5 
6 
7 
8 
SIGY 
LAMDA 
SBUCK 
POWER 
F 
F 
F 
F 
Default 
none 
0.0 
0.0 
0.0 
0.0 
0.0 
SIGY 
0.5 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
Variable 
FRACX 
FRACY 
LCTEN 
LCCOMP 
AOPT 
EBU 
DOWNSL 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.1 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
Variable 
DBAR 
FCDOW 
LCHARD 
UNITC 
UNITL 
Type 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
1.0 
1.0
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EPDAM1  EPDAM2  DRESID 
Type 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
Additional Card for AOPT ≠ 0. 
  Card 5 
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
3 
ZP 
F 
4 
A1 
F 
5 
A2 
F 
6 
A3 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
7 
8 
Additional Card for AOPT ≠ 0. 
  Card 6 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
7 
8 
BETA 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
MID 
Material identification.  A unique number has to be chosen. 
RO 
YM 
PR 
Mass density. 
Young’s Modulus 
Poisson’s Ratio 
SIGY 
Yield stress
VARIABLE   
DESCRIPTION
LAMDA 
Slenderness ratio 
SBUCK 
Initial buckling stress (should be positive) 
POWER 
Power law for Bauschinger effect (non-dimensional) 
FRACX 
FRACY 
LCTEN 
Fraction  of  reinforcement  at  this  integration  point  in  local  𝑥
direction 
Fraction  of  reinforcement  at  this  integration  point  in  local  𝑦
direction 
Optional curve providing the factor on SIGY versus plastic strain 
(tension) 
LCCOMP 
Optional  curve  providing  the  factor  on  SBUCK  versus  plastic
strain (compression) 
AOPT 
Option for local axis alignment – see material type 2 
EBU 
Optional buckling strain (if defined, overrides LAMBDA) 
DOWNSL 
Initial  down-slope  of  buckling  curve  as  a  fraction  of  YM
(dimensionless) 
DBAR 
Reinforcement bar diameter used for dowel action.  See remarks. 
FCDOW 
Concrete compressive strength used for dowel action.  See notes.
This field has units of stress 
LCHARD 
Characteristic length for dowel action (length units) 
UNITC 
UNITL 
Factor  to  convert  model  stress  units  to  MPa,  e.g.    is  model  units
are Newtons and meters, UNITC = 10−6, [UNITC] = 1/[STRESS].
Factor to convert model length units to millimeters, e.g.  if model
units are meters, UNITL = 1000, [UNITL] = 1/[LENGTH]. 
EPDAM1 
Accumulated plastic strain at which hysteretic damage begins 
EPDAM2 
Accumulated  plastic  strain  at  which  hysteretic  damage  is
complete 
DRESID 
Residual factor remaining after hysteretic damage 
XP, YP, ZP 
Coordinates of point 𝐩 for AOPT = 1 and 4
*MAY_HYSTERETIC_REINFORCEMENT 
DESCRIPTION
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2  
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3 and 4  
D1, D2, D3 
Components of vector 𝐝 for AOPT = 2  
Remarks: 
Reinforcement  is  treated  as  bars,  acting  independently  in  the  local  material  𝑥  and  𝑦 
directions.  By default, the local material 𝑥-axis is the element 𝑥-axis (parallel to the line 
from  Node  1  to  Node  2),  but  this  may  be  overridden  using  AOPT  or  Element  Beta 
angles.  
The reinforced concrete section should be defined using *INTEGRATION_SHELL, with 
some  integration  points  being  reinforcement  (using  this  material  model)  and  others 
being  concrete  (using  for  example  *MAT_CONCRETE_EC2).    By  default,  strains  in 
directions other than the local 𝑥 and 𝑦 are unresisted, so this material model should not 
be used alone (without concrete).  The area fractions of reinforcement in the local 𝑥 and 
𝑦 directions at each integration point are given by the area-weighting for the integration 
point on *INTEGRATION_SHELL times the fractions FRACX and FRACY.  
The tensile response is elastic perfectly plastic, using yield stress SIGY.  Optionally, load 
curves  may  be  used  to  describe  the  stress-strain  response  in  tension  (LCTEN)  and 
compression  (LCCOMP).    Either,  neither  or  both  curves  may  be  defined.    If  present, 
LCTEN  overrides  the  perfectly-plastic  tensile  response,  and  LCCOMP  overrides  the 
buckling curve.  The tensile and compressive plastic strains are considered independent 
of each other. 
Bar buckling may  be  defined either using the slenderness ratio LAMDA, or by setting 
the  initial  buckling  strain  EBU  and  down-slope  DOWNSL.    If  neither  are  defined,  the 
bars simply yield in compression.  If both are defined, the buckling behaviour defined 
by EBU and DOWNSL overrides LAMDA.   
The slenderness ratio LAMDA determines buckling behaviour and is defined as, 
Where, 𝑘 depends on end conditions, and 
𝐿 = unsupported length of reinforcement bars 
𝑘𝐿
, 
𝑟 = radius of gyration which for round bars is equal to (bar radius)/√2.
It  is  expected  that  users  will  determine  LAMDA  accounting  for  the  expected  crack 
spacing. 
The alternative buckling behaviour defined by EBU and DOWNSL is shown below. 
Compressive 
stress 
Yield 
-DOWNSL * YM 
-0.005 * YM 
EBU 
EBU + 0.01 
Compressive 
strain 
Reloading  after  change  of  load  direction  follows  a  Bauschinger-type  curve,  leading  to 
the hysteresis response shown below: 
*MAT_HYSTERETIC_REINFORCEMENT
)
(
 800
 600
 400
 200
 0
-200
-400
-600
-800
-30
-20
-10
 0
Strain %
 10
 20
 30
*MAY_HYSTERETIC_REINFORCEMENT 
Two  types  of  damage  accumulation  may  be  modelled.    Damage  based  on  ductility 
(strain) can be modelled using the curves LCTEN and LCCOMP – at high strain, these 
curves would show reducing stress with increasing strain.  
Damage  based  on  hysteretic  energy  accumulation  can  be  modelled  using  the 
parameters EPDAM1, EPDAM2 and DRESID.  The damage is a function of accumulated 
plastic strain: for this purpose, plastic strain increments are always treated as positive in 
both  tension  and  compression,  and  buckling  strain  also  counts  towards  the 
accumulated  plastic  strain.    The  material  has  its  full  stiffness  and  strength  until  the 
accumulated  plastic  strain  reaches  EPDAM1.    Between  plastic  strains  EPDAM1  and 
EPDAM2  the  stiffness  and  strength  fall  linearly  with  accumulated  plastic  strain, 
reaching a factor DRESID at plastic strain EPDAM2. 
Dowel Action: 
The  data  on  Card  3  defines  the  shear  stiffness  and  strength,  and  is  optional.    Shear 
resistance is assumed to occur by dowel action.  The bars bend locally to the crack and 
crush  the  concrete.    An  elastic-perfectly-plastic  relation  is  assumed  for  all  shear 
components (in-plane and through-thickness).  The assumed (smeared) shear modulus 
and yield stress applicable to the reinforcement bar cross-sectional area are as follows, 
based  on  formulae  derived  from  experimental  data  by  El-Ariss,  Soroushian,  and 
Dulacska: 
𝐺[MPa] = 8.02𝐸0.25𝐹𝑐
0.375𝐿char𝐷𝑏
0.75 
where, 
𝜏𝑦 = 1.62√𝐹𝑐𝑆𝑦 
𝐸 = steel Youngs Modulus in MPa 
𝐹𝑐 = 𝑐ompressive strength of concrete in MPa 
𝐿char = 𝑐haracteristic length of shear deformation in mm 
𝐷𝑏 = bar diameter in mm 
𝑆𝑦 = steel yield stress in MPa. 
The  input  parameters  should  be  given  in  model  units,  e.g.    DBAR  and  LCHAR  are  in 
model length units, FCDOW is in model stress units.  These will be converted internally 
using UNITL and UNITC.  
Output: 
The  output  stresses,  as  for  all  other  LS-DYNA  material  models,  are  by  default  in  the 
global  coordinate  system.    They  are  scaled  by  the  reinforcement  fractions  FRACX,
FRACY.  The plastic strain output is the accumulated plastic strain (increments always 
treated  as  positive),  and  is  the  greater  such  value  of  the  two  local  directions.    Extra 
history variables are available as follows: 
Total strain in local 𝑥 direction 
Total strain in local 𝑦 direction 
Extra variable 1:   Reinforcement stress in local 𝑥 direction (not scaled by FRACX) 
Extra variable 2:   Reinforcement stress in local 𝑦 direction (not scaled by FRACY) 
Extra variable 3:  
Extra variable 4:  
Extra variable 5:   Accumulated plastic strain in local 𝑥 direction 
Extra variable 6:   Accumulated plastic strain in local 𝑦 direction 
Extra variable 7:  
Extra variable 8:  
Extra variable 9:  
Shear stress (dowel action) in local 𝑥𝑦 
Shear stress (dowel action) in local 𝑥𝑧 
Shear stress (dowel action) in local 𝑦𝑧
*MAT_STEEL_EC3 
This is Material Type 202.  Tables and formulae from Eurocode 3 are used to derive 
the mechanical properties and their variation with temperature, although these can 
be overridden by user-defined curves.  It is currently available only for Hughes-Liu 
beam  elements.    Warning,  this  material  is  still  under  development  and  should  be 
used with caution. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
6 
7 
8 
SIGY 
F 
Default 
none 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LC_E 
LC_PR 
LC_AL 
TBL_SS 
LC_FS 
Type 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
Card 3 must be included but left blank. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density.
VARIABLE   
DESCRIPTION
E 
PR 
SIGY 
LC_E 
LC_PR 
LC_AL 
TBL_SS 
Young’s modulus – a reasonable value must be provided even if 
LC_E is also input.  See notes. 
Poisson’s ratio. 
Initial yield stress, 𝜎𝑦0. 
Optional  Loadcurve  ID:  Young’s  Modulus  vs  Temperature
(overrides E and factors from EC3). 
Optional  Loadcurve 
(overrides PR). 
ID:  Poisson’s  Ratio  vs  Temperature
Optional Loadcurve ID: alpha vs temperature (over-rides thermal 
expansion data from EC3). 
Optional  Table  ID  containing  stress-strain  curves  at  different 
temperatures (overrides curves from EC3). 
LC_FS 
Optional Loadcurve ID: failure strain vs temperature. 
Remarks: 
1.  This material model is intended for modelling structural steel in fires. 
2.  By  default,  only  E,  PR  and  SIGY  have  to  be  defined.    Eurocode  3  (EC3) 
Section 3.2 specifies the stress-strain behaviour of carbon steels at tempera-
tures  between  20C  and  1200C.    The  stress-strain  curves  given  in  EC3  are 
scaled within the material model such that the maximum stress at low tem-
peratures is SIGY, see graph below. 
3.  By  default,  the  Young’s  Modulus  E  will  be  scaled  by  a  factor  which  is  a 
function of temperature as specified in EC3.  The factor is 1.0 at low temper-
ature. 
4.  By  default,  the  thermal  expansion  coefficient  as  a  function  of  temperature 
will be as specified in EC3 Section 3.4.1.1.  
5.  LC_E, LC_PR and LC_AL are optional; they should have temperature on the 
x-axis  and  the  material  property  on  the  y-axis,  with  the  points  in  order  of 
increasing temperature.  If present (i.e.  non-zero) they over-ride E, PR, and 
the  relationships  from  EC3.    However,  a  reasonable  value  for  E  should  al-
ways be included, since these values will be used for purposes such as con-
tact stiffness calculation. 
6.  TBL_SS  is  optional.    If  present,  TBL_SS  must  be  the  ID  of  a  *DEFINE_TA-
BLE.    TBL_SS  overrides  SIGY  and  the  stress-strain  relationships  from  EC3.  
The  field  VALUE  on  the  *DEFINE_TABLE  should  contain  the  temperature
at which each stress-strain curve is applicable; the temperatures should be in 
ascending order.  The curves that follow the temperature values have (true) 
plastic strain on the x-axis, (true) yield stress on the y-axis as per other LS-
DYNA elasto-plastic material models.  As with all instances of *DEFINE TA-
BLE,  the  curves  containing  the  stress-strain  data  must  immediately  follow 
the  *DEFINE_TABLE  input  data  and  must  be  in  the  correct  order  (i.e.    the 
same order as the temperatures). 
7.  Temperature  can  be  defined  by  any  of  the  *LOAD_THERMAL  methods.  
The  temperature  does  not  have  to  start  at  zero: the  initial  temperature  will 
be  taken  as  a  reference  temperature  for  each  element,  so  non-zero  initial 
temperatures will not cause thermal shock effects. 
Figure M202-1.
*MAT_208 
This  is  Material  Type  208  for  use  with  beam  elements  using  ELFORM = 6  (Discrete 
Beam).    The  beam  elements  must  have  nonzero  initial  length  so  that  the  directions  in 
which tension and compression act can be distinguished.  See notes below. 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
4 
5 
6 
7 
8 
KAX 
KSHR 
blank 
blank 
FPRE 
TRAMP 
Type 
A8 
F 
F 
F 
F 
F 
Default 
none 
none 
0.0 
0.0 
0.0 
0.0 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCAX 
LCSHR 
FRIC 
CLEAR 
DAFAIL 
DRFAIL 
DAMAG 
T0PRE 
Type 
Default 
I 
0 
I 
0 
F 
F 
F 
F 
F 
F 
0.0 
0.0 
1.E20 
1.E20 
0.1 
0.0 
Card 3 must be included but left blank. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density.
KAX 
KSHR 
FPRE 
DESCRIPTION
Axial elastic stiffness (Force/Length units). 
Shear elastic stiffness (Force/Length units). 
Preload force. 
*MAT_BOLT_BEAM 
TRAMP 
Time duration during which preload is ramped up. 
LCAX 
LCSHR 
FRIC 
CLEAR 
DAFAIL 
DRFAIL 
Load  curve  giving  axial  load  versus  plastic  displacement  (x-
axis = displacement (length units), y-axis = force). 
Load  curve  ID  or  table  ID  giving  lateral  load  versus  plastic
displacement (x-axis - displacement (length units), y-axis - force). 
In  the  table  case,  each  curve  in  the  table  represents  lateral  load 
versus displacement at a given (current) axial load, i.e.  the values
in the table are axial forces. 
Friction  coefficient  resisting  sliding  of  bolt  head/nut  (non-
dimensional). 
Radial clearance (gap between bolt shank and the inner diameter 
of the hole)  (length units). 
Axial  tensile  displacement  at  which  failure  is  initiated  (length
units). 
Radial  displacement  at  which  failure  is  initiated  (excludes
clearance). 
DAMAG 
Failure is completed at (DAFAIL or DRFAIL)*(1+DAMAG). 
T0PRE 
Time at which preload application begins. 
Remarks: 
The element represents a bolted joint.   The nodes of the beam should be thought of as 
representing  the  points  at  the  centers  of  the  holes  in  the  plates  that  are  joined  by  the 
bolt.    It  is  expected  that  SCOOR = 0  on  *SECTION_BEAM.    This  is  contrary  to  the 
normal rules for non-zero-length discrete beams. 
The axial direction is initially the line connecting node 1 to node 2.  The axial response is 
tensile-only.    Instead  of  generating  a  compressive  axial  load,  it  is  assumed  that  a  gap 
would  develop  between  the  bolt  head  (or  nut)  and  the  surface  of  the  plate.    Contact 
between the bolted surfaces must be modelled separately, e.g.  using *CONTACT.
Curves  LCAX,  LCSHR  give  yield  force  versus  plastic  displacement  for  the  axial  and 
shear directions.  The force increments are calculated from the elastic stiffnesses, subject 
to the yield force limits given by the curves. 
CLEAR allows the bolt to slide in shear, resisted by friction between bolt head/nut and 
the surfaces of the plates, from the initial position at the center of the hole.  CLEAR is 
the  total  sliding  shear  displacement  before  contact  occurs  between  the  bolt  shank  and 
the  inside  surface  of  the  hole.    Sliding  shear  displacement  is  not  included  in  the 
displacement used for LCSHR; LCSHR is intended to represent the behaviour after the 
bolt shank contacts the edge of the hole. 
Output: beam “axial” or “X” force is the axial force in the beam.  “shear-Y” and “shear-
Z” are the shear forces. 
Other  output  is  written  to  the  d3plot  and  d3thdt  files  in  the  places  where  post-
processors  expect  to  find  the  stress  and  strain  at  the  first  two  integration  points  for 
integrated beams. 
Post-Processing data component
Actual meaning
Int.  Pt 1, Axial Stress 
Change of length 
Int Pt 1, XY Shear stress 
Sliding shear displacement in local Y 
Int Pt 1, ZX Shear stress 
Sliding shear displacement in local Z 
Int Pt 1, Plastic strain 
Resultant shear sliding displacement 
Int Pt 1, Axial strain 
Axial plastic displacement 
Int.  Pt 2, Axial Stress 
Int Pt 2, XY Shear stress 
Int Pt 2, ZX Shear stress 
Int Pt 2, Plastic strain 
Int Pt 2, Axial strain 
Shear  plastic  displacement  excluding 
sliding 
- 
- 
- 
-
*MAT_SPR_JLR 
This  is  Material  Type  211.    This  material  model  was  written  for  Self-Piercing  Rivets 
(SPR) connecting aluminium sheets.  It intended that each SPR is modelled by a single 
hexahedral (8-node solid) element, fixed to the sheet either by direct meshing or by tied 
contact.  Pre- and post-processing methods are the same as for solid-element Spotwelds 
using *MAT_SPOTWELD.  On *SECTION_SOLID, set ELFORM = 1. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
Default 
none 
none 
none 
none 
5 
6 
7 
8 
HELAS 
TELAS 
F 
0 
F 
0 
Cards 2 and 3 define” Head” end of SPR inputs 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCAXH 
LCSHH 
LCBMH 
SFAXH 
SFSHH 
SFBMH 
Type 
F 
F 
F 
Default 
none 
none 
none 
  Card 3 
1 
2 
3 
F 
1 
4 
F 
1 
5 
F 
1 
6 
Variable 
DFAKH 
DFSHH 
RFBMH  DMFAXH  DMFSHH  DMFBMH 
7 
8 
Type 
F 
F 
F 
F 
F 
F 
Default 
see 
notes 
see 
notes 
see 
notes 
0.1 
0.1 
0.1
Cards 4 and 5 define “Tail” end of SPR inputs 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCAXT 
LCSHT 
LCBMT 
SFAXT 
SFSHT 
SBFMT 
Type 
F 
F 
F 
Default 
none 
none 
none 
  Card 5 
1 
2 
3 
F 
1 
4 
F 
1 
5 
F 
1 
6 
Variable 
DFAXT 
DFSHT 
RFBMT 
DFMAXT  DMFSHT  DMFBMT 
7 
8 
Type 
F 
F 
F 
F 
F 
F 
Default 
see 
notes 
see 
notes 
see 
notes 
0.1 
0.1 
0.1 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus, used only for contact stiffness calculation. 
Poisson’s ratio, used only for contact stiffness calculation. 
HELAS 
SPR head end behaviour flag: 
EQ.0.0: Nonlinear. 
EQ.1.0: Elastic (Use first two points on load curves). 
TELAS 
SPR tail end behaviour flag: 
EQ.0.0: Nonlinear. 
EQ.1.0: Elastic (Use first two points on load curves). 
LCAXH 
Load  curve  ID,  see  *DEFINE_CURVE,  giving  axial  force  versus 
deformation (head).
LCSHH 
*MAT_SPR_JLR 
DESCRIPTION
Load  curve  ID,  see  *DEFINE_CURVE,  giving  shear  force  versus 
deformation (head). 
LCBMH 
Load  curve  ID,  see  *DEFINE_CURVE,  giving  moment  versus 
rotation (head). 
SFAXH 
Scale factor on axial force from curve LCAXH. 
SFSHH 
Scale factor on shear force from curve LCSHH. 
SFBMH 
Scale factor on bending moment from curve LCBMH. 
DFAXH 
Optional displacement to start of softening in axial load (head). 
DFSHH 
Optional displacement to start of softening in shear load (head). 
RFBMH 
Optional rotation (radians) to start of bending moment softening
(head). 
DMFAXH 
Scale factor on DFAXH. 
DMFSHH 
Scale factor on FFSHH. 
DMFBMH 
Scale factor on RFBMH. 
LCAXT 
LCSHT 
LCBMT 
Load  curve  ID,  see  *DEFINE_CURVE,  giving  axial  force  versus 
deformation (tail). 
Load  curve  ID,  see  *DEFINE_CURVE,  giving  shear  force  versus 
deformation (tail). 
Load  curve  ID,  see  *DEFINE_CURVE,  giving  moment  versus 
rotation (tail). 
SFAXT 
Scale factor on axial force from curve LCAXT. 
SFSHT 
Scale factor on shear force from curve LCSHT. 
SFBMT 
Scale factor on bending moment from curve LCBMT. 
DFAXT 
Optional displacement to start of softening in axial load (tail). 
DFSHT 
Optional displacement to start of softening in shear load (tail). 
RFBMT 
Optional rotation (radians) to start of bending moment softening
(tail).
VARIABLE   
DESCRIPTION
DMFAXT 
Scale factor on DFAXT. 
DMFSHT 
Scale factor on FFSHT. 
DMFBMT 
Scale factor on RFBMT. 
Remarks: 
1. 
“Head” is the end of the SPR that fully perforates a sheet.  “Tail” is the end that 
is embedded within the thickness of a sheet. 
2.  E and PR are used only to calculate contact stiffness.  They are not used by the 
material model. 
3.  Deformation  is  in  length  units  and  is  on  the  x-axis.    Force  is  on  the  y-axis.  
Rotation is in radians, on the x-axis.  Moment is on the y-axis. 
4.  All the loadcurves are expected to start at (0,0).  “Deformation” means the total 
deformation  including  both  elastic  and  plastic  components,  and  similarly  for 
rotation. 
5.  A “high tide” algorithm is used to determine the deformation or rotation to be 
used as the x-axis of the loadcurves when looking up the current yield force or 
moment.    The  “high  tide”  is  the  greatest  displacement  or  rotation that  has  oc-
curred so far during the analysis. 
6.  The  first  two  points  of  the  curve  define  the  elastic  stiffness,  which  is  used  for 
unloading.  
7. 
If HELAS > 0, the remainder of the head loadcurves after the first two points is 
ignored  and  no  softening  or  failure  occurs.    Similarly  for  TELAS  and  the  tail 
loadcurves. 
8.  The sheet planes are defined at the head by the quadrilateral defined by nodes 
N1-N2-N3-N4 of the solid element; and at the tail by the quadrilateral defined 
by nodes N5-N6-N7-N8.  
9.  The  tail  of  the  SPR  is  defined  as  a  point  in  the  tail  sheet  plane,  initially  at  the 
centre of the element face.  The head of the SPR is initially at the centre of the 
head sheet plane.  Thus the axis of the SPR would typically be coincident with 
the solid element local z-axis if the solid is a cuboid.  It is the user’s responsibil-
ity to ensure that each solid element is oriented correctly.
10.  During  the  analysis,  the  head  and  tail  will  always  remain  in  the  plane  of  the 
sheet,  but  may  move  away  from  the  centres  of  the  sheet  planes  if  the  shear 
forces in these planes are sufficient. 
11.  The SPR axis is defined as the line joining the tail to the head. 
12.  Axial deformation is defined as change of length of the line between the tail and 
head of the SPR.  This line also defines the direction in which the axial force is 
applied. 
13.  Shear deformation is defined as motion of the tail and head points, in the sheet 
planes.  This deformation is not necessarily perpendicular to axial deformation.  
Shear  forces  in  these  planes  are  controlled  by  the  loadcurves  LCSHT  and 
LCSHH. 
14.  Rotation  at  the tail  is defined  as  rotation  of the  tail-to-head  line relative to the 
normal  of  the  tail  sheet  plane;  and  for  the  head,  relative  to  the  normal  of  the 
head sheet plane. 
15.  Displacement/rotation to start of softening (DFAXH, DFSHH, etc): if non-zero 
values are input, these must be within the abcissa values of the relevant curve, 
such that the curve force/moment value is greater than zero at the defined start 
of softening.  
16.  Although  ELFORM = 1  is  used  in  the  input  data,  *MAT_SPR_JLR  is  really  a 
separate  unique  element  formulation.    The  usual  stress/force  and  hourglass 
calculations are bypassed, and deformations and nodal forces are calculated by 
a  method  unique  to  *MAT_SPR_JLR;  for  example,  a  single  *MAT_SPR_JLR 
element can carry bending loads.  
17.  *HOURGLASS inputs are irrelevant to *MAT_SPR_JLR. 
18.  It is essential that the nodes N1 to N4 are fixed to the head sheet (e.g.  by direct 
meshing or tied contact): the element has no stiffness to resist relative motion of 
nodes N1 to N4 in the plane of the head sheet.  Similarly, nodes N5 to N8 must 
be fixed to the tail sheet. 
19.  Output  to  SWFORC  file  works  in  the  same  way  as  for  Spotwelds.    Although 
inside  the  material  model  the  loadcurves  LCSHT  and  LCSHH  control  “shear” 
forces in the sheet planes, in the SWFORC file the quoted shear force is the force 
normal to the axis of the SPR.  
20.  Before  an  element  fails,  it  enters  a  “softening”  regime  in  which  the  forces, 
moments  and  stiffnesses  are  ramped  down  as  displacement  increases  (this 
avoids  sudden  shocks  when  the  element  is  deleted).    For  example,  for  axial 
loading  at  the  head,  softening  begins  when  the  maximum  axial  displacement
exceeds  DFAXH.    As  the  displacement  increases  beyond  that  point,  the 
loadcurve  will  be  ignored  for  that  deformation  component.    The  forces,  mo-
ments  and  stiffnesses  are  ramped  down  linearly  with  increasing  displacement 
and  reach  zero  at  displacement = DFAXH*(1+DMFAXH)  when  the  element  is 
deleted.    The  softening  factor  scales  all  the  force  and  moment  components  at 
both  head  and  tail.    Thus  all  the  force  and  moment  components  are  reduced 
when any one displacement component enters the softening regime.  For exam-
ple  if  DFAXT = 3.0mm,  and  DMFAXT = 0.1,  then  softening  begins  when  axial 
displacement of the head reaches 3.0mm and final failure occurs at 3.3mm. 
21.  If the inputs DFAXT etc are left blank or zero, they will be calculated internally 
as follows: 
a)  Final  failure  will  occur  at  the  displacement  or  rotation  (DFAIL)  at  which 
the loadcurve reaches zero (determined if necessary by extrapolation from 
the last two points). 
b)  Displacement  or  rotation  at  which  softening  begins  is  then  back-
calculated, for example DFAXT = DFAIL/(1+DMGAXT). 
c)  If DMGAXT was left blank or zero, it defaults to 0.1. 
d)  If the loadcurve does not drop to zero, and the final two points have a ze-
ro or positive gradient, no failure or softening will be caused by that dis-
placement component. 
22.  Output stresses (in the d3plot and time-history output files) are set to zero.  
23.  The  output  variable  “displacement  ratio”  (or  rotation  ratio  for  bending),  R,  is 
defined as follows.  See also the Figure M211-1. 
a)  R = 0 to 1: The maximum force or moment on the input curve has not yet 
been reached.  R is proportional to the maximum force or moment reached 
so far, with 1.0 being the point of maximum force or moment on the input 
curve.  
b)  R = 1 to 2: The element has passed the point of maximum force but has not 
yet  entered  the  softening  regime.    R  rises  linearly  with  displacement  (or 
rotation) from 1.0 when maximum force occurs to 2.0 when softening be-
gins.  
c)  R = 2 to 3: Softening is occurring.  R rises linearly with displacement from 
2.0 at the onset of softening to 3.0 when the element is deleted.
Force or 
moment
R=1.0
R=1.0
R=2.0
R=3.0
Linear ramp-
down replaces 
the input 
loadcurve in 
the softening 
regime
R=0.0
DF
DMF
Displacement 
or Rotation
Figure  [M211-1].    Output  variable  “displacement  ratio”  (or  rotation  ratio  for
bending) 
24.  Displacement  (or  Rotation)  Ratio  is  calculated  separately  for  axial,  shear  and 
bending at the tail and head .  The output 
listed  by  post-processors  as  “plastic  strain”  is  actually  the  maximum  displace-
ment  or  rotation  ratio  of  any  displacement  or  rotation  component  at  head  or 
tail.  This same variable is also output as “Failure” in the spotweld data in the 
swforc file (or the swforc section of the binout file). 
25.  Output extra history variables: 
1Failure time (used for SWFORC file) 
2(Softening factor used internally to prevent abrupt failure) 
3Displacement ratio – axial, head 
4Displacement ratio – axial, tail  
5Displacement ratio – shear, head 
6Displacement ratio – shear, tail 
7Rotation ratio – bending, head  
8Rotation ratio – bending, tail  
9(Used for SWFORC output) 
10Shear force in “beam” x-axis  
11 Shear force in “beam” y-axis  
12Axial force in “beam” z-axis (along “beam”)  
13Moment about “beam” x-axis at head 
14Moment about “beam” y-axis at head 
15Moment about “beam” z-axis at head (torsion – should be zero)  
16“Beam” length  
17Moment about “beam” x-axis at tail 
18Moment about “beam” y-axis at tail 
19Moment about “beam” z-axis at tail (torsion – should be zero)
20Isoparametric coordinate of head of “beam” (s) 
21Isoparametric coordinate of head of “beam” (t) 
22Isoparametric coordinate of tail of “beam” (s) 
23Isoparametric coordinate of tail of “beam” (t) 
24Timestep 
25Plastic displacement, axial, head  
26Plastic displacement, axial, tail  
27Plastic rotation, head  
28Plastic rotation, tail 
29Plastic displacement, shear in sheet axes, head 
30Plastic displacement, shear in sheet axes, tail  
31Beam x-axis (global x component) 
32Beam x-axis (global y component) 
33Beam x-axis (global z component) 
34Shear displacement, local x, head  
35Shear displacement, local y, head 
36Shear displacement, local x, tail 
37Shear displacement, local y, tail 
38Total displacement – axial 
39Current rotation (radians)  – head, local X direction 
40Current rotation (radians)  – head, local Y direction 
41Current rotation (radians)  – tail, local X direction 
42Current rotation (radians)  – tail, local Y direction
*MAT_DRY_FABRIC 
This  is  Material  Type  214.    This  material  model  can  be  used  to  model  high  strength 
woven  fabrics,  such  as  Kevlar®  49,  with  transverse  orthotropic  behavior  for  use  in 
structural systems where high energy absorption is required (Bansal et al., Naik et al., 
Stahlecker  et  al.).    The  major  applications  of  the  model  are  for  the  materials  used  in 
propulsion engine containment system, body armor and personal protections. 
Woven  dry  fabrics  are  described  in  terms  of  two  principal  material  directions, 
longitudinal  warp    and  transverse  fill  yarns.    The  primary  failure  mode  in  these 
materials  is  the  breaking  of  either  transverse  or  longitudinal  yarn.    An  equivalent 
continuum  formulation  is  used  and  an  element  is  designated  as  having  failed  when  it 
reaches some critical value for strain in either directions.  A linearized approximation to 
a  typical  stress-strain  curve  is  shown  in  Figure  M214-1,  and  to  a  typical  engineering 
shear stress-strain curve is shown in the  figure corresponding to the GABi field in the 
variable list.  Note that the principal directions are labeled 𝑎 for the warp and 𝑏 for the 
fill, and the direction 𝑐 is orthogonal to 𝑎 and 𝑏. 
The material model is available for membrane elements and it is recommended to use a 
double precision version of LS-DYNA. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
EA 
F 
3 
4 
EB 
F 
4 
Variable 
GBC 
GCA 
GAMAB1  GAMAB2 
F 
2 
Type 
F 
  Card 3 
1 
Variable 
AOPT 
Type 
F 
F 
F 
3 
XP 
F 
4 
YP 
F 
5 
6 
7 
8 
GAB1 
GAB2 
GAB3 
F 
5 
5 
ZP 
F 
F 
6 
6 
A1 
F 
F 
7 
7 
A2 
F 
8 
8 
A3
Variable 
1 
V1 
Type 
F 
  Card 5 
1 
2 
V2 
F 
2 
3 
V3 
F 
3 
4 
D1 
F 
4 
5 
D2 
F 
5 
6 
D3 
F 
6 
*MAT_214 
7 
8 
BETA 
F 
7 
8 
Variable 
EACRF 
EBCRF 
EACRP 
EBCRP 
Type 
Remarks 
F 
2 
  Card 6 
1 
F 
2 
2 
F 
F 
3 
4 
5 
6 
7 
8 
Variable 
EASF 
EBSF 
EUNLF 
ECOMF 
EAMAX 
EBMAX 
SIGPOST 
Type 
Remarks 
F 
2 
  Card 7 
1 
F 
2 
2 
F 
2 
3 
F 
2 
4 
F 
F 
F 
5 
6 
7 
8 
Variable 
CCE 
PCE 
CSE 
PSE 
DFAC 
EMAX 
EAFAIL 
EBFAIL 
Type 
Remarks 
F 
1 
F 
1 
F 
1 
F 
1 
F 
3 
F 
4 
F 
4 
F 
4 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Continuum equivalent mass density.
SIGPOST
E [ A / B ] C
E C O M P
E[A/B]
[
/
]
E[A/B]SF
These strains values
depend on the particular
unloading path.
Pre-peak 
linear 
behavior
Post-peak 
linear 
behavior
Crimp
Unloading & 
Reloading
Post-peak
non-linear
behavior
[
/
]
[
/
Strain
]
Failure
Strain
Figure  M214-1.    Stress  –  Strain  curve  for  *MAT_DRY_FABRIC.    This  curve
models the force-response in the longitudinal and transverse directions. 
  VARIABLE   
DESCRIPTION
EA 
EB 
GABi / 
GAMABi 
GBC 
GCA 
AOPT 
Modulus  of  elasticity  in  the  longitudinal  (warp)  direction,  which 
corresponds to the slope of segment AB in Figure  M214-1. 
Modulus  of  elasticity  in  the  transverse  (fill)  direction,  which
corresponds to the slope of segment of AB Figure  M214-1. 
Shear  stress-strain  behavior  is 
modeled  as  piecewise  linear 
in  three  segments.    See  the 
figure  to  the  right.    The  shear 
moduli  GABi  correspond  to 
the  slope  of  the  ith  segment.  
The  start  and  end  points  for 
the  segments  are  specified  in 
the GAMAB[1-2] fields. 
𝐺𝑏𝑐, Shear modulus in 𝑏𝑐 direction. 
𝐺𝑐𝑎, Shear modulus in 𝑐𝑎 direction. 
G A B 2
GAB1
Shear
Strain
Material axes option.  See *MAT_OPTIONTROPIC_ELASTIC for a 
more complete description: 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element  nodes  1,  2,  and  4,  as  with  *DEFINE_COORDI-
NATE_NODES,  and  then  rotated  about  the  element
normal by an angle BETA.
VARIABLE   
DESCRIPTION
EQ.2.0: globally  orthotropic  with  material  axes  determined  by 
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally orthotropic material axes determined by rotating
the material axes about the element normal by an angle,
BETA, from a line in the plane of the element defined by 
the  cross  product  of  the  vector  v  with  the  element  nor-
mal. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).    Available  in  R3  version  of  971 
and later. 
XP, YP, ZP 
Components of vector 𝐱. 
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3. 
D1, D2, D3 
Components of vector 𝐝 for AOPT = 2. 
BETA 
EACRF 
Material angle in degrees for AOPT = 0 and 3, may be overridden 
on the element card, see *ELEMENT_SHELL_BETA. 
Factor  for  crimp  region  modulus  of  elasticity  in  longitudinal 
direction : 
𝐸𝑎,crimp = 𝐸𝑎,crimpfac𝐸,
𝐸𝑎,crimpfac = EACRF 
EBCRF 
Factor  for  crimp  region  modulus  of  elasticity  in  transverse 
direction : 
𝐸𝑏,crimp = 𝐸𝑏,crimpfac𝐸,
𝐸𝑏,crimpfac = EBCRF 
EACRP 
Crimp strain in longitudinal direction : 
𝜀𝑎,crimp
EBCRP 
Crimp strain in transverse direction : 
𝜀𝑏,crimp
EASF 
*MAT_DRY_FABRIC 
DESCRIPTION
Factor  for  post-peak  region  modulus  of  elasticity  in  longitudinal
direction : 
𝐸𝑎,soft = 𝐸𝑎,softfac𝐸,
𝐸𝑎,softfac = EASF 
EBSF 
Factor  for  post-peak  region  modulus  of  elasticity  in  transverse
direction : 
𝐸𝑏,soft = 𝐸𝑏,softfac𝐸,
𝐸𝑏,softfac = EBSF 
EUNLF 
Factor for unloading modulus of elasticity : 
𝐸unload = 𝐸unloadfac𝐸,
𝐸unloadfac = EUNLF 
ECOMPF 
Factor  for  compression  zone  modulus  of  elasticity  : 
𝐸comp = 𝐸compfac𝐸,
𝐸compfac = ECOMPF 
EAMAX 
Strain at peak stress in longitudinal direction : 
𝜀𝑎,max
EBMAX 
Strain at peak stress in transverse direction : 
𝜀𝑏,𝑚𝑎𝑥
SIGPOST 
Stress  value  in  post-peak  region  at  which  nonlinear  behavior 
begins : 
𝜎post
CCE 
PCE 
CSE 
PSE 
Strain  rate  parameter 𝐶,  Cowper-Symonds  factor  for  modulus.    If 
zero,  rate effects are not considered. 
Strain  rate  parameter  𝑃,  Cowper-Symonds  factor  for  modulus.    If 
zero,  rate effects are not considered. 
Strain rate parameter 𝐶, Cowper-Symonds factor for stress to peak 
/ failure.  If zero, rate effects are not considered. 
Strain rate parameter 𝑃, Cowper-Symonds factor for stress to peak 
/ failure.  If zero, rate effects are not considered. 
DFAC 
Damage factor: 
𝑑fac
VARIABLE   
DESCRIPTION
EMAX 
Erosion strain of element: 
𝜀max
EAFAIL 
Erosion strain in longitudinal direction : 
𝜀𝑎,fail
EBFAIL 
Erosion strain in transverse direction : 
𝜀𝑏,fail
Remarks: 
1.  Strain  rate  effects  are  accounted  for  using  a  Cowper-Symonds  model  which 
scales the stress according to the strain rate: 
𝛔adj = 𝛔 (1 +
)
. 
𝜀̇
In the above equation 𝛔 is the quasi-static stress,  𝛔adj is the adjusted stress ac-
counting for strain rate 𝜀̇, 𝐶 (CCE) and 𝑃 (PCE) are the Cowper-Symonds factors 
and have to be determined experimentally for each material. 
The  model  captures  the  non-linear  strain  rate  effects  in  many  materials.    With 
its  less  than  unity  exponent,  1/𝑝 ,  this  model  captures  the  rapid  increase  in 
material properties at low strain rate, while increasing less rapidly at very high 
strain rates.  Because stress is a function of strain rate the elastic stiffness also is: 
𝐄adj = 𝐄 (1 +
)
𝜀̇
where 𝐄adj is the adjusted elastic stiffness.  Additionally, the strains to peak and 
strains to failure are assumed to follow a Cowper-Symonds model with, possibly 
different, constants 
𝜀adj = ε (1 +
𝑃𝑠 
)
𝜀̇
𝐶𝑠
where, 𝜀adj is the adjusted effective strain to peak stress or strain to failure, and 
𝐶𝑠 and 𝑃𝑠 are CSE and PSE respectively. 
2.  When  strained  beyond  the  peak  stress,  the  stress  decreases  linearly  until  it 
attains  a  value  equal  to  SIGPOST,  at  which  point  the  stress-strain  relation  be-
comes nonlinear.  In the non-linear region the stress is given by
𝜎 =   𝜎post
⎢⎡1 − (
⎣
𝜀 − 𝜀[𝑎/𝑏],post
𝜀[𝑎/𝑏],fail − 𝜀[𝑎/𝑏],post
)
𝑑fac
⎥⎤  
⎦
where  𝜎post  and  𝜀post  are,  respectively,  the  stress  and  strain  demarcating  the 
onset  of  nonlinear  behavior.    The  value  of  SIGPOST  is  the  same  in  both  the 
transverse  and  longitudinal  directions,  whereas  𝜀a,post  and  𝜀b,post  depend  on 
direction and are derived internally from EASF, EBSF, and SIGPOST.  The fail-
ure strain, 𝜀[𝑎/𝑏],fail, specifies the onset of failure and differs in the longitudinal 
and  transverse  directions.    Lastly  the  exponent,  𝑑fac,  determines  the  shape  of 
nonlinear stress-strain curve between 𝜀post and 𝜀[𝑎 𝑏⁄ ],fail. 
3.  The element is eroded if either (a) or (b) is satisfied: 
a)  𝜀𝑎 >   𝜀𝑎,fail and 𝜀𝑏 >   𝜀𝑏,fail 
b)  𝜀𝑎 >   𝜀max and 𝜀𝑏 >   𝜀max.
*MAT_215 
This  is  Material  Type  215.    A  micromechanical  material  that  distinguishes  between  a 
fiber/inclusion  and  a  matrix  material,  developed  by  4a  engineering  GmbH.    It  is 
available for the explicit code for shell, thick shell and solid elements. Useful hints and 
input example can be found in [1].  More theory and application notes will be provided 
soon in [2].  
The material is intended for anisotropic composite materials, especially for short (SFRT) 
and long fiber thermoplastics (LFRT).  The matrix behavior is described by an isotropic 
elasto-viscoplastic  von  Mises  model.    The  fiber/inclusion  behavior  is  transversal 
isotropic  elastic.    This  also  allows  to  use  this  material  model  for  classical  endless  fiber 
composites. 
The  inelastic  homogenization  for  describing  the  composite  deformation  behavior  is 
based on: 
•Mori Tanaka Meanfield Theory [3,4] 
•ellipsoidal inclusions using Eshelby´s solution [5,6] 
•orientation averaging [7] 
•a  linear  fitted  closure  approximation  to  determine  the  4th  order  fiber  orientation 
tensor out of the user provided 2nd order fiber orientation tensor. 
The  core  functionality  to  calculate  the  thermo-elastic  composite  properties  can  be  also 
found in the software product 4a micromec [8]. 
Failure/Damage of the composite can be currently considered by  
•a ductile damage initiation and evolution model for the matrix (DIEM) 
•fiber failure may be considered with a maximum stress criterion. 
More details on the material characterization can be found in [9] and [10]. 
The (fiber) orientation can be defined either for the whole material using CARD 2 and 3 
or elementwise using *ELEMENT_(T)SHELL_BETA or *ELEMENT_SOLID_ORTHO. 
The  mechanical  properties  of  SFRT  and  LFRT  in  injection  molded  parts  are  highly 
influenced through the manufacturing process.  By mapping the fiber orientation from 
the process simulation to the structural analysis the local anisotropy can be considered 
[11,12].  The  fiber  orientation,  length  and  volume  fraction  can  therefore  as  well  be 
defined for each integration point by using *INITIAL_STRESS_(T)SHELL(SOLID) [2].  
Details on the history variables that can be initialized (Extravars.  9-18) can be found in 
the output section.
*MAT_4A_MICROMEC 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
MMOPT 
BUPD 
FAILM 
FAILF 
NUMINT 
Type 
A8 
F 
F 
F 
F 
F 
Default 
none 
0.0 
0.01 
0.0 
0.0 
1.0 
Parameter for fiber orientation (may be overwritten by 
*INITIAL_STRESS_SHELL/SOLID) 
  Card 2 
1 
2 
Variable 
AOPT 
MACF 
Type 
F 
Default 
0.0 
  Card 3 
Variable 
1 
V1 
Type 
F 
F 
0 
2 
V2 
F 
3 
XP 
F 
4 
YP 
F 
5 
ZP 
F 
6 
A1 
F 
7 
A2 
F 
8 
A3 
F 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
7 
8 
BETA 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0
1 
2 
Variable 
FVF 
Type 
F 
3 
FL 
F 
4 
FD 
F 
*MAT_215 
5 
6 
7 
8 
A11 
A22 
F 
F 
Default 
0.0 
0.0 
1.0 
1.0 
0.0 
Parameter for fiber/inclusion material 
  Card 5 
1 
Variable 
ROF 
Type 
F 
2 
EL 
F 
3 
ET 
F 
4 
5 
6 
7 
8 
GLT 
PRTL 
PRTT 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
2 
3 
4 
5 
6 
7 
8 
  Card 6 
Variable 
1 
XT 
Type 
F 
Default 
0.0 
Parameter for matrix material 
  Card 7 
1 
Variable 
ROM 
Type 
F 
2 
E 
F 
3 
PR 
F 
Default 
0.0 
0.0 
0.0 
SLIMXT 
NCYRED 
F 
F 
0.0 
10 
4 
5 
6 
7
Card 8 
1 
2 
3 
4 
5 
Variable 
SIGYT 
ETANT 
Type 
F 
F 
EPS0 
F 
6 
C 
F 
7 
8 
Default 
0.0 
0.0 
0.0 
0.0 
  Card 9 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCIDT 
LCDI 
UPF 
Type 
Default 
F 
0 
  VARIABLE   
MID 
F 
0 
F 
0.0 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
MMOPT 
Option to define micromechanical material behavior  
EQ.0.0: elastic 
EQ.1.0: elastic-plastic 
BUPD 
Tolerance for update of Strain-Concentration Tensor
VARIABLE   
FAILM 
DESCRIPTION
Opion for matrix failure – ductile DIEM-Model.  
 based on 
stress  triaxiality  and  a  linear  damage  evolution  (DETYP.EQ.0)
type) 
LT.0:  |FAILM| Effective plastic matrix strain at failure.  When 
the matrix plastic strain reaches this value, the element is
deleted from the calculation.  
EQ.0: only visualization (triaxiality of matrix stresses) 
EQ.1: active DIEM (triaxiality of matrix stresses) 
EQ.10: only visualization (triaxiality of composite stresses) 
EQ.11: active DIEM (triaxiality of composite stresses) 
FAILF 
Option for fiber failure  
EQ.0: only visualization (equivalent fiber stresses) 
EQ.1: active (equivalent fiber stresses) 
NUMINT 
Number of failed integration points prior to element deletion. 
LT.0.0:  Only  for  shells.    |NUMINT|  is  the  percentage  of
integration points which must exceed the failure criterion
before  element  fails.    For  shell  formulations  with  4  inte-
gration  points  per  layer,  the  layer  is  considered  failed  if
any of the integration points in the layer fails. 
 Parameter for fiber orientation 
AOPT 
See *MAT_002 (fiber orientation information may be overwritten
using *INITIAL_STRESS_(T)SHELL/SOLID) 
MACF 
Material axes change flag for solid elements: 
EQ.1: No change, default, 
EQ.2: switch material axes a and b, 
EQ.3: switch material axes a and c, 
EQ.4: switch material axes b and c. 
XP, YP, ZP 
Define coordinates of point p for AOPT = 1 and 4. 
A1, A2, A3 
Define components of vector a for AOPT = 2.
*MAT_4A_MICROMEC 
DESCRIPTION
V1, V2, V3 
Define components of vector v for AOPT = 3 and 4. 
D1, D2, D3 
Define components of vector d for AOPT = 2. 
BETA 
Material  angle  in  degrees  for  AOPT = 3,  may  be  overwritten  on 
the element card, see  
*ELEMENT_(T)SHELL_BETA or *ELEMENT_SOLID_ORTHO. 
FVF 
Fiber-Volume-Fraction  
GT.0: Fiber-Volume-Fraction 
LT.0: |FVF| Fiber-Mass-Fraction 
FL 
FD 
A11 
A22 
Fiber length - if FD = 1 then FL = aspect ratio (may be overwritten 
by *INITIAL_STRESS_(T)SHELL/SOLID) 
Fiber diameter (may be overwritten by 
*INITIAL_STRESS_(T)SHELL/SOLID) 
Value of first principal fiber orientation (may be overwritten by 
*INITIAL_STRESS_(T)SHELL/SOLID). 
Value of second principal fiber orientation (may be overwritten 
by *INITIAL_STRESS_(T)SHELL/SOLID). 
Parameter for fiber/inclusion material 
ROF 
Mass density of fiber 
EL 
ET 
GLT 
PRTL 
PRTT 
XT 
EL, Young’s modulus of fiber – longitudinal direction. 
ET, Young’s modulus of fiber – transverse direction. 
GLT, Shear modulus LT 
 TL, Poisson’s ratio TL 
 TT, Poisson’s ratio TT 
Fiber tensile strength – longitudinal direction. 
SLIMXT 
Factor  to  determine  the  minimum  stress  limit  in  the  fiber  after 
stress maximum (fiber tension)
NCYRED 
Number  of  cycles  for  stress  reduction  from  maximum  to
minimum (fiber tension) 
Parameter for matrix material 
ROM 
Mass density of matrix. 
E 
PR 
SIGYT 
ETANT 
EPS0 
C 
LCIDT 
Young’s modulus of matrix. 
Poisson’s ratio of matrix. 
Yield stress of matrix in tension 
Tangent  modulus  of  matrix  in  tension,  ignore  if  (LCST.GT.0.)  is
defined. 
Quasi-static  threshold  strain  rate  (Johnson-Cook  model)  for  bi-
linear hardening 
Johnson-Cook constant for bi-linear hardening 
Load  curve  ID  or  Table  ID  for  defining  effective  stress  versus
effective  plastic  strain  in  tension  of  matrix  material  (Table  to
include strain-rate effects, viscoplastic formulation) 
LCDI 
Damage initiation parameter (ductile) 
shells:  Load  curve  ID  representing  plastic  strain  at  onset  of 
damage as function of stress triaxiality. 
or 
Table ID representing plastic strain at onset of damage as
function of stress triaxiality and plastic strain rate. 
solids:  Load  curve  ID  representing  plastic  strain  at  onset  of 
damage as function of stress triaxiality. 
or 
Table ID representing plastic strain at onset of damage as
function of stress triaxiality and lode angle. 
or 
Table3D ID representing plastic strain at onset of damage
as  function  of  stress  triaxiality,  lode  angle  and  plastic 
strain rate.
UPF 
Damage evolution parameter  
𝑝 
GT.0.0: plastic displacement at failure, 𝑢𝑓
LT.0.0: |UPF| is a table ID for 𝑢𝑓
𝑝 as a function of triaxiality and
 damage 
Output: 
“Plastic Strain” is the equivalent plastic strain in the matrix.  
Extra history variables may be requested for (t)shell (NEIPS) and solid (NEIPH) 
elements  on *DATABASE_EXTENT_BINARY. Extra history variables 1-8 are 
intended for post processing, 9-18 for initialization with 
*INITIAL_STRESS_(T)SHELL/SOLID.  They have the following meaning: 
  Extravar. 
DESCRIPTION
1 
2 
3 
4 
5 
6 
7 
8 
effs - equivalent plastic strain rate of matrix 
eta - triaxiality of matrix ...  = −
q 
xi - lode parameter of matrix ...  = −
27∙J3
2∙q  
dM - Damage initiation d of matrix (Ductile Criteria) 
DM - Damage evolution D of matrix  
RFF - Fiber reserve factor 
DF- Fiber damage variable 
Currently unused 
  Extravar. 
DESCRIPTION 
9 
10 
11 
12 
13 
14 
15 
16 
A11 - fiber orientation first principal value 
A22 - fiber orientation first second value 
q1/q11 
q2/q12 
-/q13 
-/q31 
-/q32 
-/q33
17 
18 
FVF- Fiber-Volume-Fraction 
FL- Fiber length 
References: 
 [1]   Reithofer, P., et.  al, *MAT_4A_MICROMEC – micro mechanic based material model,  14th German 
LS-DYNA Conference (2016), Bamberg 
 [2]   Reithofer, P., et.  al, *MAT_4A_MICROMEC – Theory and application notes, 11th European LS-
DYNA Conference (2017), Salzburg 
 [3]   Mori, T., Tanaka, K., Average Stress in Matrix and Average elastic Energy of Materials with 
misfitting Inclusions, Acta Metallurgica, Vol.21, pp.571-574, (1973). 
 [4]   Tucker  Ch.    L.    III,  Liang  Erwin:  Stiffness  Predictions  for  Unidirectional  Short-Fibre  Composites: 
Review and Evaluation, Composites Science and Technology, 59, (1999) 
 [5]   Maewal A., Dandekar D.P.: Effective Thermoelastic Properties of Short-Fibre Composites, Acta 
Mechanica, 66, (1987) 
 [6]   Eshelby, J.  D., The determination of the elastic field of an ellipsoidal inclusion, and related 
problems, Proceedings of the Royal Society, London, Vol.A, No241, pp.376-396, (1957). 
 [7]   Mlekusch, B., Kurzfaserverstärkte Thermoplaste, Dissertation, Montanuniversität Leoben (1997) 
 [8]   http://micromec.4a.co.at 
 [9]   Reithofer, P.  et.  al: Material characterization of composites using micro mechanic models as key 
enabler, NAFEMS DACH, Bamberg 2016 
[10]   http://impetus.4a.co.at  
[11]   Reithofer, P.  et.  al: Short and long fiber reinforced thermoplastics material models in LS-DYNA, 
10th European LS-DYNA Conference, Würzburg 2015 
[12]   http://fibermap.4a.co.at
*MAT_ELASTIC_PHASE_CHANGE 
This  is  Material  Type  216,  a  generalization  of  Material  Type  1,  for  which  material 
properties change on an element-by-element basis upon crossing a plane in space.  This 
is an isotropic hypoelastic material and is available only for shell element types. 
5 
6 
7 
8 
5 
6 
7 
8 
Phase 1 Properties. 
  Card 1 
1 
2 
Variable 
MID 
RO1 
Type 
A8 
F 
3 
E1 
F 
4 
PR1 
F 
Default 
none 
none 
none 
0.0 
Phase 2 Properties. 
  Card 1 
1 
2 
Variable 
Type 
RO2 
F 
3 
E2 
F 
4 
PR2 
F 
Default 
none 
none 
0.0 
Transformation Plane Card. 
  Card 2 
Variable 
1 
X1 
Type 
F 
2 
Y1 
F 
3 
Z1 
F 
4 
X2 
F 
5 
Y2 
F 
6 
Z2 
F 
7 
8 
THKFAC 
F 
Default 
none 
none 
none 
none 
none 
none 
1.0
VARIABLE   
DESCRIPTION
MID 
ROi 
Ei 
PRi 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density for phase i. 
Young’s modulus for phase i. 
Poisson’s ratio for phase i. 
X1, Y1, Z1 
Coordinates of a point on the phase transition plane. 
Coordinates  of  a  point  that  defines  the  exterior  normal  with  the
first point. 
Scale  factor  applied  to  the  shell  thickness  after  the  phase
transformation. 
X2, Y2, Z2 
THKFAC 
Phases: 
The  material  properties  for  each  element  are  initialized  using  the  data  for  the  first 
phase.    After  the  center  of the  element  passes  through  the transition  plane  defined  by 
the two points, the material properties are irreversibly changed to the second phase. 
The plane is defined by two points.  The first point, defined by the coordinates X1, Y1, 
and Z1, lies on the plane.  The second point, defined by the coordinates X2, Y2, and Z2, 
define  the  exterior  normal  as  a  unit  vector  in  the  direction  from  the  first  point  to  the 
second point. 
Remarks: 
This  hypoelastic  material  model  may  not  be  stable  for  finite  (large)  strains.      If  large 
strains  are  expected,  a  hyperelastic  material  model,  e.g.,  *MAT_002  or  *MAT_217, 
would be more appropriate.
*MAT_OPTIONTROPIC_ELASTIC_PHASE_CHANGE 
This  is  Material  Type  217  a  generalization  of  Material  Type  2  for  which  material 
properties change on an element-by-element basis upon crossing a plane in space. 
This  material  is  valid  only  for  shells.    The  stress  update  is  incremental  and  the  elastic 
constants are formulated in terms of Cauchy stress and true strain. 
Available options include: 
ORTHO 
ANISO 
such that the keyword cards appear: 
*MAT_ORTHOTROPIC_ELASTIC_PHASE_CHANGE or MAT_217 
(9 cards follow) 
*MAT_ANISOTROPIC_ELASTIC_PHASE_CHANGE or MAT_217_ANIS 
(11 cards follow) 
Orthotropic Card 1 (phase 1).  Card 1 for ORTHO keyword option for phase 1. 
  Card 1 
1 
2 
Variable 
MID 
RO1 
Type 
A8 
F 
3 
EA 
F 
4 
EB 
F 
5 
EC 
F 
6 
7 
8 
PRBA 
PRCA 
PRCB 
F 
F 
F 
Orthotropic Card 2 (phase 1).  Card 2 for ORTHO keyword option for phase 1. 
  Card 2 
1 
2 
3 
4 
Variable 
GAB 
GBC 
GCA 
AOPT1 
Type 
F 
F 
F 
F 
5 
G 
F 
6 
7 
8 
SIGF
Anisotropic Card 1 (phase 1).  Card 1 for ANISO keyword option for phase 1. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
RO2 
C111 
C121 
C221 
C131 
C231 
C331 
Type 
A8 
F 
F 
F 
F 
F 
F 
F 
Anisotropic Card 2 (phase 1).  Card 2 for ANISO keyword option for phase 1. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
C141 
C241 
C341 
C441 
C151 
C251 
C351 
C451 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Anisotropic Card 3 (phase 1).  Card 3 for ANISO keyword option for phase 1. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
C551 
C161 
C261 
C361 
C461 
C561 
C661 
AOPT1 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Local Coordinate System Card 1 (phase 1).  Required for  all keyword options 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
XP1 
YP1 
ZP1 
A11 
A21 
A31 
MACF 
IHIS 
Type 
F 
F 
F 
F 
F 
F 
I 
F 
Local Coordinate System Card 2 (phase 1).  Required for  all keyword options 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
V11 
V21 
V31 
D11 
D21 
D31 
BETA1 
REF 
Type 
F 
F 
F 
F 
F 
F 
F
Orthotropic Card 3 (phase 2).  Card 1 for ORTHO keyword option phase 2. 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
EA2 
EB2 
EC2 
PRBA2 
PRCA2 
PRCB2 
F 
F 
F 
F 
F 
F 
Orthotropic Card 4 (phase 2).  Card 2 for ORTHO keyword option phase 2. 
  Card 7 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
GAB2 
GBC2 
GCA2 
Type 
F 
F 
F 
Anisotropic Card 4 (phase 2).  Card 1 for ANISO keyword option for phase 2. 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
C112 
C122 
C222 
C132 
C232 
C332 
F 
F 
F 
F 
F 
F 
Anisotropic Card 5 (phase 2).  Card 2 for ANISO keyword option for phase 2. 
  Card 7 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
C142 
C242 
C342 
C442 
C152 
C252 
C352 
C452 
Type 
F 
F 
F 
F 
F 
F 
F
Anisotropic Card 6 (phase 2).  Card 3 for ANISO keyword option for phase 2. 
  Card 8 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
C552 
C162 
C262 
C362 
C462 
C562 
C662 
Type 
F 
F 
F 
F 
F 
F 
F 
Local Coordinate System Card 1 (phase 2).  Required for  all keyword options 
  Card 9 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
XP2 
YP2 
ZP2 
A12 
A22 
A32 
MACF2 
Type 
F 
F 
F 
F 
F 
F 
I 
Local Coordinate System Card 2 (phase 2).  Required for  all keyword options 
  Card 10 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
V12 
V22 
V32 
D12 
D22 
D32 
BETA2 
Type 
F 
F 
F 
F 
F 
F 
F 
Definition of transformation plane Card. 
  Card 11 
Variable 
1 
X1 
Type 
F 
2 
Y1 
F 
3 
Z1 
F 
4 
X2 
F 
5 
Y2 
F 
6 
Z2 
F 
7 
8 
THKFAC 
F 
Default 
none 
none 
none 
none 
none 
none 
1.0 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified.
ROi 
Mass density for phase i. 
Define for the ORTHO option only: 
EAi 
EBi 
ECi 
PRBAi 
PRCAi 
PRCBi 
GABi 
GBCi 
GCAi 
𝐸𝑎, Young’s modulus in 𝑎-direction for phase i. 
𝐸𝑏, Young’s modulus in 𝑏-direction for phase i. 
𝐸𝑐,  Young’s  modulus  in  𝑐-direction  phase  i  (nonzero  value 
required but not used for shells). 
𝜈𝑏𝑎, Poisson’s ratio in the 𝑏𝑎 direction for phase i. 
𝜈𝑐𝑎, Poisson’s ratio in the ca direction for phase i. 
𝜈𝑐𝑏, Poisson’s ratio in  the 𝑐𝑏 direction for phase i. 
𝐺𝑎𝑏, shear modulus in  the ab direction for phase i. 
𝐺𝑏𝑐, shear modulus in the 𝑏𝑐 direction for phase i. 
𝐺𝑐𝑎, shear modulus in the 𝑐𝑎 direction for phase i. 
Due to symmetry define the upper triangular Cij’s for the ANISO option only: 
C11i 
C12i 
⋮ 
C66i 
The 1,1 term in the 6 × 6 anisotropic constitutive matrix for phase 
i.  Note that 1 corresponds to the 𝑎 material direction 
The 1,2 term in the 6 × 6 anisotropic constitutive matrix for phase 
i.  Note that 2 corresponds to the 𝑏 material direction 
⋮
The 6,6 term in the 6 × 6 anisotropic constitutive matrix for phase 
i. 
Define AOPT for both options: 
AOPTi 
Material axes option for phase i, see Figure M2-1. 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element  nodes  as  shown  in  part  (a)  of  Figure  M2-1. 
The a-direction is from node 1 to node 2 of the element.
The  b-direction  is  orthogonal  to  the  a-direction  and  is 
in  the  plane  formed  by  nodes  1,  2,  and  4.    When  this
option is used  in two-dimensional planar and axisym-
metric  analysis,  it  is  critical  that  the  nodes  in  the  ele-
ment definition be numbered counterclockwise for this
option to work correctly. 
EQ.1.0: locally orthotropic with material axes determined by a
point  in  space  and  the  global  location  of  the  element
center;  this  is  the  𝐚-direction.    This  option  is  for  solid 
elements only. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by 
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  𝐯  with  the 
element  normal.    The  plane  of  a  solid  element  is  the
midsurface between the inner surface and outer surface
defined by the first four nodes and the last four nodes 
of the connectivity of the element, respectively. 
EQ.4.0: locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector  𝐯,  and 
an originating point, 𝐏, which define the centerline ax-
is.  This option is for solid elements only. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
G 
Shear  modulus  for  frequency  independent  damping.    Frequency
independent  damping  is  based  of  a  spring  and  slider  in  series.
The critical stress for the slider mechanism is SIGF defined below.
For  the  best  results,  the  value  of  G  should  be  250-1000  times 
greater than SIGF.  This option applies only to solid elements. 
SIGF 
Limit stress for frequency independent, frictional, damping. 
XPi, YPi, ZPi 
Define coordinates of the ith phase’s point 𝐩 for AOPT = 1 and 4. 
A1i, A2i, A3i 
Define components of the ith phase’s vector 𝐚 for AOPT = 2. 
MACFi 
Material axes change flag for brick elements in phase i: 
EQ.1: No change, default, 
EQ.2: switch material axes 𝑎 and 𝑏,
EQ.3: switch material axes 𝑎 and 𝑐, 
EQ.4: switch material axes 𝑏 and 𝑐. 
IHIS 
Flag  for  anisotropic  stiffness  terms  initialization  (for  solid
elements only). 
EQ.0: C11, C12, … from Cards 1, 2, and 3 are used. 
EQ.1: C11,  C12,  …  are  initialized  by  *INITIAL_STRESS_SOL-
ID’s history data. 
V1i, V2i, V3i 
Define components of the ith phase’s vector 𝐯 for AOPT = 3 and 4.
D1i, D2i, D3i 
Define components of the ith phase’s vector 𝐝 for AOPT = 2. 
BETAi 
REFi 
Material  angle  of  ith  phase  in  degrees  for  AOPT = 3,  may  be 
overridden  on  the  element  card,  see  *ELEMENT_SHELL_BETA 
or *ELEMENT_SOLID_ORTHO. 
Use  reference  geometry  to  initialize  the  stress  tensor  for  the  ith
phase.  The reference  geometry is defined by the keyword: *INI-
TIAL_FOAM_REFERENCE_GEOMETRY  . 
EQ.0.0: off, 
EQ.1.0: on. 
X1, Y1, Z1 
Coordinates of a point on the phase transition page. 
Coordinates  of  a  point  that  defines  the  exterior  normal  with  the
first point. 
Scale  factor  applied  to  the  shell  thickness  after  the  phase
transformation. 
X2, Y2, Z2 
THKFAC 
Phases: 
The  material  properties  for  each  element  are  initialized  using  the  data  for  the  first 
phase.    After  the  center  of the  element  passes  through  the transition  plane  defined  by 
the two points, the material properties are irreversibly changed to the second phase. 
The plane is defined by two points.  The first point, defined by the coordinates X1, Y1, 
and Z1, lies on the plane.  The second point, defined by the coordinates X2, Y2, and Z2, 
define  the  exterior  normal  as  a  unit  vector  in  the  direction  from  the  first  point  to  the 
second point.
Material Formulation: 
The material law that relates stresses to strains is defined as: 
𝐂 = 𝐓T𝐂𝐿𝐓 
where 𝐓 is a transformation matrix, and 𝐂𝐿 is the constitutive matrix defined in terms of 
the  material  constants  of  the  orthogonal  material  axes,  {𝐚, 𝐛, 𝐜}.    The  inverse  of    𝐂𝐿for 
the orthotropic case is defined as: 
−1 =
𝐂𝐿
𝐸𝑎
𝜐𝑎𝑏
𝐸𝑎
𝜐𝑎𝑐
𝐸𝑎
−
−
−
−
𝜐𝑏𝑎
𝐸𝑏
𝐸𝑏
𝜐𝑏𝑐
𝐸𝑏
−
−
𝜐𝑐𝑎
𝐸𝑐
𝜐𝑐𝑏
𝐸𝑐
𝐸𝑐
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
𝐺𝑎𝑏
𝐺𝑏𝑐
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
𝐺𝑐𝑎⎦
Where, 
𝜐𝑎𝑏
𝐸𝑎
=
𝜐𝑏𝑎
𝐸𝑏
,
𝜐𝑐𝑎
𝐸𝑐
=
𝜐𝑎𝑐
𝐸𝑎
,
𝜐𝑐𝑏
𝐸𝑐
=
𝜐𝑏𝑐
𝐸𝑏
. 
The frequency independent damping is obtained by having a spring and slider in series 
as shown in the following sketch:  
friction
This  option  applies  only  to  orthotropic  solid  elements  and  affects  only  the  deviatoric 
stresses. 
The procedure for describing the principle material directions is explained for solid and 
shell elements for this material model and other anisotropic materials.  We will call the 
material  direction  the  {𝐚, 𝐛, 𝐜}  coordinate  system.    The  AOPT  options  illustrated  in 
Figure  M2-1  can  define  the  {𝐚, 𝐛, 𝐜}  system  for  all  elements  of  the  parts  that  use  the 
material, but this is not the final material direction.  There {𝐚, 𝐛, 𝐜} system defined by the 
AOPT options may be offset by a final rotation about the 𝐜-axis.  The offset angle we call 
BETA. 
For  solid  elements,  the  BETA  angle  is  specified  in  one  of  two  ways.    When  using 
AOPT = 3,  the  BETA  parameter  defines  the  offset  angle  for  all  elements  that  use  the 
material.    The  BETA  parameter  has  no  meaning  for  the  other  AOPT  options.
Alternatively, a BETA angle can be defined for individual solid elements as described in 
remark  5  for  *ELEMENT_SOLID_ORTHO.    The  beta  angle  by  the  ORTHO  option  is 
available for all values of AOPT, and it overrides the BETA angle on the *MAT card for 
AOPT = 3. 
The  directions  determined  by  the  material  AOPT  options  may  be  overridden  for 
individual  elements  as  described  in  remark  3  for  *ELEMENT_SOLID_ORTHO.  
However,  be  aware  that  for  materials  with  AOPT = 3,  the  final  {𝐚, 𝐛, 𝐜}  system  will  be 
the  system  defined  on  the  element  card  rotated  about  𝐜-axis  by  the  BETA  angle 
specified on the *MAT card. 
There  are  two  fundamental  differences  between  shell  and  solid  element  orthotropic 
materials.    First,  the  𝐜-direction  is  always  normal  to  a  shell  element  such  that  the  𝐚-
direction  and  𝐛-directions  are  within  the  plane  of  the  element.    Second,  for  some 
anisotropic materials, shell elements may have unique fiber directions within each layer 
through the thickness of the element so that a layered composite can be modeled with a 
single element. 
When  AOPT = 0  is  used  in  two-dimensional  planar  and  axisymmetric  analysis,  it  is 
critical that the nodes in the element definition be numbered counterclockwise for this 
option to work correctly. 
Because shell elements have their 𝐜-axes defined by the element normal, AOPT = 1 and 
AOPT = 4  are  not  available  for  shells.    Also,  AOPT = 2  requires  only  the  vector  𝐚  be 
defined since 𝐝 is not used.  The shell procedure projects the inputted 𝐚-direction onto 
each element surface. 
Similar  to  solid  elements,  the  {𝐚, 𝐛, 𝐜}  coordinate  system  determined  by  AOPT  is  then 
modified  by  a  rotation  about  the 𝐜-axis  which  we  will  call  𝜙.    For  those  materials  that 
allow a unique rotation angle for each integration point through the element thickness, 
the rotation angle is calculated by 
𝜙𝑖 = 𝛽 + 𝛽𝑖 
where  𝛽  is  a  rotation  for  the  element,  and  𝛽𝑖  is  the  rotation  for  the  i’th  layer  of  the 
element.  The 𝛽 angle can be input using the BETA parameter on the *MAT data, or will 
be  overridden  for  individual  elements  if  the  BETA  keyword  option  for  *ELEMENT_-
SHELL  is  used.    The  𝛽𝑖  angles  are  input  using  the  ICOMP = 1  option  of  *SECTION_-
SHELL or with *PART_COMPOSITE.  If 𝛽 or 𝛽𝑖 is omitted, they are assumed to be zero. 
All  anisotropic  shell  materials  have  the  BETA  option  on  the  *MAT  card  available  for 
both AOPT = 0 and AOPT = 3, except for materials 91 and 92 which have it available for 
all values of AOPT, 0, 2, and 3. 
All  anisotropic  shell  materials  allow  an  angle  for  each  integration  point  through  the 
thickness, 𝛽𝑖, except for materials 2, 86, 91, 92, 117, 130, 170, 172, and 194.
This discussion of material direction angles in shell elements also applies to thick shell 
elements  which  allow  modeling  of  layered  composites  using  *INTEGRATION_SHELL 
or *PART_COMPOSITE_TSHELL.
*MAT_MOONEY-RIVLIN_PHASE_CHANGE 
This  is  Material  Type  218,  a  generalization  of  Material  Type  27,  for  which  material 
properties change on an element-by-element basis upon crossing a plane in space. 
Phase 1 Card 1. 
  Card 1 
1 
2 
3 
Variable 
MID 
RO1 
PR1 
Type 
A8 
F 
F 
4 
A1 
F 
5 
B1 
F 
6 
REF 
F 
7 
8 
Phase 1 Card 2. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SGL1 
SW1 
ST1 
LCID1 
Type 
F 
F 
F 
F 
Phase 2 Card 1. 
  Card 3 
1 
2 
3 
Variable 
RO2 
PR2 
Type 
F 
F 
4 
A2 
F 
5 
B2 
F 
6 
7 
8 
Phase 2 Card 2. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SGL2 
SW2 
ST2 
LCID2 
Type 
F 
F 
F
Transformation Plane Card. 
  Card 5 
Variable 
1 
X1 
Type 
F 
2 
Y1 
F 
3 
Z1 
F 
4 
X2 
F 
5 
Y2 
F 
6 
Z2 
F 
7 
8 
THKFAC 
F 
Default 
none 
none 
none 
none 
none 
none 
1.0 
  VARIABLE   
DESCRIPTION
MID 
ROi 
PRi 
Ai 
Bi 
REF 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density for phase i. 
Poisson’s  ratio  (value  between  0.49  and  0.5  is  recommended,
smaller values may not work) where i indicates the phase. 
Constant  for  the  ith  phase,  see  literature  and  equations  defined 
below. 
Constant  for  the  ith  phase,  see  literature  and  equations  defined 
below. 
Use  reference  geometry  to  initialize  the  stress  tensor.    The
reference geometry is defined by the keyword:*INITIAL_FOAM_-
REFERENCE_GEOMETRY . 
EQ.0.0: off, 
EQ.1.0: on.
gauge
length
Force
AA
Δ gauge length
Section AA
thickness
width
Figure M218-1.  Uniaxial specimen for experimental data 
If A = B = 0.0, then a least square fit is computed from tabulated uniaxial data via a 
load curve.  The following information should be defined: 
  VARIABLE   
DESCRIPTION
SGLi 
SWi 
STi 
LCIDi 
Specimen gauge length 𝑙0 for the ith phase, see Figure M218-1. 
Specimen width for the ith phase, see Figure M218-1. 
Specimen thickness for the ith phase, see Figure M218-1. 
Curve ID for the ith phase, see *DEFINE_CURVE, giving the force 
versus  actual  change  Δ𝐿  in  the  gauge  length.    See  also  Figure 
M218-2 for an alternative definition. 
X1, Y1, Z1 
Coordinates of a point on the phase transition plane. 
X2, Y2, Z2 
THKFAC 
Coordinates  of  a  point  that  defines  the  exterior  normal  with  the
first point. 
Scale  factor  applied  to  the  shell  thickness  after  the  phase
transformation.
Phases: 
The  material  properties  for  each  element  are  initialized  using  the  data  for  the  first 
phase.    After  the  center  of the  element  passes  through  the transition  plane  defined  by 
the two points, the material properties are irreversibly changed to the second phase. 
The plane is defined by two points.  The first point, defined by the coordinates X1, Y1, 
and Z1, lies on the plane.  The second point, defined by the coordinates X2, Y2, and Z2, 
define  the  exterior  normal  as  a  unit  vector  in  the  direction  from  the  first  point  to  the 
second point. 
Material Formulation: 
The strain energy density function is defined as: 
𝑊 = 𝐴(𝐼 − 3) + 𝐵(𝐼𝐼 − 3) + 𝐶(𝐼𝐼𝐼−2 − 1) + 𝐷(𝐼𝐼𝐼 − 1)2 
where 
𝐶  =  0.5 𝐴  +  𝐵 
𝐷 =
𝐴(5𝜐 − 2) + 𝐵(11𝜐 − 5)
2(1 − 2𝜐)
𝜈  =  Poisson’s ratio 
2(𝐴 + 𝐵)   = shear modulus of linear elasticity 
𝐼, 𝐼𝐼, 𝐼𝐼𝐼 =  invariants of right Cauchy-Green Tensor C. 
The  load  curve  definition  that  provides  the  uniaxial  data  should  give  the  change  in 
gauge  length,  Δ𝐿,  versus  the  corresponding  force.    In  compression  both  the  force  and 
the  change  in  gauge  length  must  be  specified  as  negative  values.    In  tension  the  force 
and  change  in  gauge  length  should  be  input  as  positive  values.    The  principal  stretch 
ratio in the uniaxial direction, 𝜆1, is then given by 
𝐿0 + Δ𝐿
𝐿0
𝜆1 =
with 𝐿0 being the initial length and 𝐿 being the actual length.
applied force
initial area
=
A0
change in gauge length
gauge length
=
∆L
Figure  M218-2    The  stress  versus  strain  curve  can  used  instead  of  the  force
versus  the  change  in  the  gauge  length  by  setting  the  gauge  length,  thickness,
and  width  to  unity  (1.0)  and  defining  the  engineering  strain  in  place  of  the
change  in  gauge  length  and  the  nominal  (engineering)  stress  in  place  of  the
force.  *MAT_077_O is a better alternative for fitting data resembling the curve
above.    *MAT_027  will  provide  a  poor  fit  to  a  curve  that  exhibits  a  strong
upturn in slope as strains become large. 
Alternatively,  the  stress  versus  strain  curve  can  also  be  input  by  setting  the  gauge 
length, thickness, and width to unity (1.0) and defining the engineering strain in place 
of the change in gauge length and the nominal (engineering) stress in place of the force, 
see Figure M218-1. 
The least square fit to the experimental data is performed during the initialization phase 
and is a comparison between the fit and the actual input is provided in the d3hsp file.  
It is a good idea to visually check to make sure it is acceptable.  The coefficients 𝐴 and 𝐵 
are  also  printed  in  the  output  file.    It  is  also  advised  to  use  the  material  driver   for checking out the material model.
*MAT_219 
This  is  material  type  219.    This  material  model  is  the  second  generation  of  the  UBC 
Composite  Damage  Model  (CODAM2)  for  brick,  shell,  and  thick  shell  elements 
developed  at  The  University  of  British  Columbia.    The  model  is  a  sub-laminate-based 
continuum damage mechanics model for fiber reinforced composite laminates made up 
of  transversely  isotropic  layers.    The  material  model  includes  an  optional  non-local 
averaging and element erosion. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
EA 
F 
4 
EB 
F 
5 
6 
7 
8 
PRBA 
PRCB 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
5 
Variable 
GAB 
NLAYER 
R1 
Type 
F 
Default 
none 
  Card 3 
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
3 
ZP 
F 
I 
0 
4 
A1 
F 
6 
R2 
F 
F 
0.0 
0.0 
5 
A2 
F 
6 
A3 
F 
7 
8 
NFREQ 
I 
0 
7 
AOPT 
I 
0 
8 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
*MAT_CODAM2 
7 
8 
BETA 
MACF 
F 
I 
0 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Angle Cards.  For each of the NLAYER layers specify on angle.  Include as many cards 
as needed to set NLAYER values. 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ANGLE1 
ANGLE2 
ANGLE3 
ANGLE4 
ANGLE5 
ANGLE6 
ANGLE7 
ANGLE8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IMATT 
IFIBT 
ILOCT 
IDELT 
SMATT 
SFIBT 
SLOCT 
SDELT 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 7 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IMATC 
IFIBC 
ILOCC 
IDELC 
SMATC 
SFIBC 
SLOCC 
SDELC 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none
Card 8 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ERODE 
ERPAR1 
ERPAR2 
RESIDS 
Type 
Default 
I 
0 
F 
F 
none 
none 
F 
0 
  VARIABLE   
DESCRIPTION
MID 
RO 
EA 
EB 
PRBA 
PRCB 
GAB 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
𝐸𝑎,  Young’s  modulus  in  𝑎-direction.    This  is  the  modulus  along 
the direction of fibers. 
𝐸𝑏,  Young’s  modulus  in  𝑏-direction.    This  is  the  modulus 
transverse to fibers. 
𝜈𝑏𝑎, Poisson’s ratio, 𝑏𝑎 (minor in-plane Poisson’s ratio). 
𝜈𝑐𝑏, Poisson’s ratio, 𝑐𝑏 (Poisson’s ratio in the plane of isotropy). 
𝐺𝑏𝑎, Shear modulus, 𝑎𝑏 (in-plane shear modulus). 
NLAYER 
Number of layers in the sub-laminate excluding symmetry.  As an 
example, in a [0/45/-45/90]3s, NLAYER = 4.  
R1 
R2 
NFREQ 
Non-local averaging radius. 
Currently not used. 
Number  of  time  steps  between  update  of  neighbor  list  for
nonlocal smoothing. 
EQ.0: Do only one search at the start of the calculation 
XP, YP, ZP 
Coordinates of point 𝐩 for AOPT = 1 and 4. 
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2.
AOPT 
*MAT_CODAM2 
DESCRIPTION
Material  axes  option  : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES, and then, for shells only, rotated about
the shell element normal by an angle BETA. 
EQ.1.0: locally orthotropic with material axes determined by a 
point  in  space  and  the  global  location  of  the  element
center;  this  is  the  𝑎-direction.    This  option  is  for  solid 
elements only. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  𝐯  with  the 
element normal. 
EQ.4.0: locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector  𝐯,  and 
an originating point, 𝐩, which define the centerline ax-
is.  This option is for solid elements only. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID 
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR). 
V1, V2, V3 
Components of vector v for AOPT = 3 and 4. 
D1, D2, D3 
Components of vector d for AOPT = 2. 
BETA 
Material  angle  in  degrees  for  AOPT = 0  (shells  only)  and 
AOPT = 3.    BETA  be  overridden  on  the  element  card,  see  *ELE-
MENT_SHELL_BETA or *ELEMENT_SOLID_ORTHO.
VARIABLE   
DESCRIPTION
MACF 
Material axes change flag for brick elements: 
EQ.1: No change, default, 
EQ.2: switch material axes 𝑎 and 𝑏, 
EQ.3: switch material axes 𝑎 and 𝑐, 
EQ.4: switch material axes 𝑏 and 𝑐. 
ANGLEi 
Rotation  angle  in  degrees  of  layers  with  respect  to  the  material
axes.   Input one for each layer.  
IMATT 
IFIBT 
ILOCT 
IDELT 
SMATT 
SFIBT 
SLOCT 
SDELT 
IMATC 
IFIBC 
Initiation  strain  for  damage  in  matrix  (transverse)  under  tensile 
condition. 
Initiation  strain  for  damage  in  the  fiber  (longitudinal)  under
tensile condition. 
Initiation  strain  for  the  anti-locking  mechanism.    This  parameter 
should  be  equal  to  the  saturation  strain  for  the  fiber  damage
mechanism under tensile condition.  
Not working in the current version.  Can be used for visualization
purpose only. 
Saturation  strain  for  damage in  matrix  (transverse)  under  tensile
condition. 
Saturation  strain  for  damage  in  the  fiber  (longitudinal)  under
tensile condition. 
Saturation  strain  for  the  anti-locking  mechanism  under  tensile 
condition. 
  The  recommended  value  for  this  parameter  is 
(ILOCT+0.02).  
Not working in the current version.  Can be used for visualization
purpose only.  
Initiation  strain  for  damage 
compressive condition. 
in  matrix  (transverse)  under
Initiation  strain  for  damage  in  the  fiber  (longitudinal)  under
compressive condition.
ILOCC 
IDELC 
SMATC 
SFIBC 
SLOCC 
SDELC 
ERODE 
*MAT_CODAM2 
DESCRIPTION
Initiation  strain  for  the  anti-locking  mechanism.    This  parameter 
should  be  equal  to  the  saturation  strain  for  the  fiber  damage
mechanism under compressive condition.  
Initiation  strain  for  delamination.    Not  working  in  the  current
version.  Can be used for visualization purpose only. 
Saturation  strain  for  damage  in  matrix  (transverse)  under
compressive condition. 
Saturation  strain  for  damage  in  the  fiber  (longitudinal)  under 
compressive condition. 
Saturation  strain 
for 
compressive  condition. 
parameter is (ILOCC + 0.02).  
the  anti-locking  mechanism  under 
  The  recommended  value  for  this
Delamination strain.  Not working in the current version.  Can be
used for visualization purpose only.  
Erosion Flag  
EQ.0: Erosion is turned off. 
EQ.1: Non-local strain based erosion criterion. 
EQ.2: Local strain based erosion criterion. 
EQ.3: Use both ERODE = 1 and ERODE = 2 criteria. 
ERPAR1 
ERPAR2 
The  erosion  parameter  #1  used  in  ERODE  types  1  and  3.
ERPAR1>=1.0 and the recommended value is ERPAR1 = 1.2. 
The  erosion  parameter  #2  used  in  ERODE  types  2  and  3.    The
recommended  value  is  five  times  SLOCC  defined  in  cards  7  and 
8. 
RESIDS 
Residual strength for layer damage 
Model Description: 
CODAM2  is  developed  for  modeling  the  nonlinear,  progressive  damage  behavior  of 
laminated  fiber-reinforced  plastic  materials.    The  model  is  based  on  the  work  by 
(Forghani, 2011; Forghani et al.  2011a; Forghani et al.  2011b) and is an extension of the 
original model, CODAM (Williams et al.  2003).
Briefly,  the  model  uses  a  continuum  damage  mechanics  approach  and  the  following 
assumptions have been made in its development: 
1.  The  material  is  an  orthotropic  medium  consisting  of  a  number  of  repeating 
units  through  the  thickness  of  the  laminate,  called  sub-laminates.    e.g.  
[0/±45/90] in a [0/±45/90]8S laminate. 
2.  The  nonlinear  behavior  of  the  composite  sub-laminate  is  only  caused  by 
damage  evolution.    Nonlinear  elastic  or  plastic  deformations  are  not  consid-
ered. 
Formulation: 
The in-plane secant stiffness of the damaged laminate is represented as the summation 
of the effective contributions of the layers in the laminate as shown. 
𝐀𝑑 = ∑ 𝑡𝑘𝚻𝑘
T𝐐𝑘
𝑑𝚻𝑘 
𝑑 is the in-plane secant 
where 𝚻𝑘 is the transformation matrix for the strain vector, and 𝐐𝑘
stiffness of kth layer in the principal orthotropic plane, and  𝑡𝑘 is the thickness of the  kth 
layer of an 𝑛-layered laminate. 
A  physically-based  and  yet  simple  approach  has  been  employed  here  to  derive  the 
damaged  stiffness  matrix.    Two  reduction  coefficients,  𝑅𝑓    and  𝑅𝑚,  that  represent  the 
reduction of stiffness in the longitudinal (fiber) and transverse (matrix) directions have 
been  employed.    The  shear  modulus  has  also  been  reduced  by  the  matrix  reduction 
parameter.    The  major  and  minor  Poisson’s  ratios  have  been  reduced  by  𝑅𝑓 and 𝑅𝑚re-
spectively.  A sub-laminate-level reduction, 𝑅𝐿, is incorporated to avoid spurious stress 
locking in the damaged zone.  This would lead to an effective reduced stiffness matrix 
𝑑. The reduction coefficients are equal to 1 in the undamaged condition and gradually 
𝐐𝑘
decrease to 0 for a saturated damage condition. 
𝐐𝑘
𝑑 = 𝑅𝐿
𝜈12𝜈21
𝐸1
(𝑅𝑓 )
(𝑅𝑚)
𝜈12𝐸2
⎡
⎢
1 − (𝑅𝑓 )
⎢
⎢
(𝑅𝑚)
(𝑅𝑓 )
⎢
⎢
⎢
(𝑅𝑚)
1 − (𝑅𝑓 )
⎢
⎢
⎢
⎣
𝜈12𝜈21
𝜈12𝐸2
(𝑅𝑚)
(𝑅𝑚)
𝐸2
(𝑅𝑓 )
1 − (𝑅𝑓 )
(𝑅𝑚)
(𝑅𝑚)
1 − (𝑅𝑓 )
𝜈12𝜈21
𝜈12𝜈21
(𝑅𝑚)
𝑑T
= 𝐐𝑘
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
𝐺12⎦
where 𝐸1, 𝐸2, 𝜈12, 𝜈21, and 𝐺12 are the elastic constants of the lamina.
*MAT_CODAM2 
In CODAM2, the evolution of damage mechanisms are expressed in terms of equivalent 
strain  parameters.    The  equivalent  strain  function  that  governs  the  fiber  stiffness 
reduction parameter is written in terms of the longitudinal normal strains by 
eq = 𝜀11,𝑘,
𝜀𝑓 ,𝑘
𝑘 = 1, . . . , 𝑛 
The equivalent strain function that governs the matrix stiffness reduction parameter is 
written  in  an  interactive  form  in  terms  of  the  transverse  and  shear  components  of  the 
local strain. 
eq = sign(𝜀22,𝑘)√(𝜀22,𝑘)2 + (
𝜀𝑚,𝑘
𝛾12,𝑘
)
,
𝑘 = 1, . . . , 𝑛 
The sign of the transverse normal strain plays a very important role in the initiation and 
growth of damage since it indicates the compressive or tensile nature of the transverse 
stress.    Therefore,  the  equivalent  strain  for  the  matrix  damage  carries  the  sign  of  the 
transverse normal strain. 
Evolution  of  the  overall  damage  mechanism  (anti-locking)  is  written  in  terms  of  the 
maximum principal strains. 
eq = max[prn(ε)] 
𝜀𝐿
Within  the  framework  of  non-local  strain-softening  formulations  adopted  here,  all 
damage  modes,  be  it  intra-laminar  (i.e.    fiber  and  matrix  damage)  or  overall  sub-
laminate modes are considered to be a function of the non-local (averaged) equivalent 
strain defined as: 
eq = ∫ 𝜀𝛼
𝜀̅𝛼
Ω𝐗
eq(𝐱)𝑤𝛼(𝐗 − 𝐱)𝑑Ω
where  the  subscript  𝛼  denotes  the  mode  of  damage:  fiber  (𝛼 = 𝑓 )  and  matrix  (𝛼 = 𝑚) 
damage  in  each  layer,  𝑘,  within  the  sub-laminate  or  associated  with  the  overall  sub-
eq and 
laminate, namely, locking (𝛼 = 𝐿).  Thus, for a given sub-laminate with n layers,𝜀𝛼
eq are vectors of size 2𝑛  + 1.  𝐗 represents the position vector of the original point of 
𝜀̅𝛼
interest  and  𝐱  denotes  the  position  vector  of  all  other  points  (Gauss  points)  in  the 
averaging zone denoted by Ω.  In classical isotropic non-local averaging approach, this 
zone  is  taken  to  be  spherical  (or  circular  in  2D)  with  a  radius  of  r  (named  R1  in  the 
material  input  card).    The  parameter,  𝑟,  which  affects  the  size  of  the  averaging  zone, 
introduces  a  length  scale  into the  model  that  is  linked  directly to  the  predicted  size  of 
the damage zone.  Averaging is done with a bell-shaped weight function, 𝑤𝛼, evaluated 
by 
𝑤𝛼 =
⎢⎡1 − (
⎣
)
⎥⎤
⎦
ε i
ε s
eq
(a)
(b)
Figure  M219-1.    illustrations  of  (a)  damage  parameter  and  (b)  reduction
parameter. 
where 𝑑 is the distance from the integration point of interest to another integration point 
with the averaging zone. 
The damage parameters, 𝜔, are calculated as a function of the corresponding averaged 
equivalent  strains.    In  CODAM2  the  damage  parameters  are  assumed  to  grow  as  a 
hyperbolic  function  of  the  damage  potential  (non-local  equivalent  strains)  such  that 
when  used  in  conjunction  with  stiffness  reduction  factors  that  vary  linearly  with  the 
damage parameters they result in a linear strain-softening response (or a bilinear stress-
strain curve) for each mode of damage 
eq∣ − 𝜀𝛼
𝑖 )
𝑖 )
𝑠 − 𝜀𝛼
eq∣ − 𝜀𝛼
∣𝜀̅𝛼
(∣𝜀̅𝛼
(𝜀𝛼
𝑖 > 0 
𝜔𝛼 =
,
𝜀𝛼
𝑒𝑞∣
∣𝜀̅𝛼
where  superscripts  𝑖  and  𝑠  denote,  respectively,  the  damage  initiation  and  saturation 
values of the strain quantities to which they are assigned.  The initiation and saturation 
parameters  are  defined  in  material  cards  #6  and  #7.    Damage  is  considered  to  be  a 
monotonically increasing function of time, t, such that 
𝜔𝛼 = max
τ<t
(𝜔𝛼
𝜏) 
where 𝜔𝛼
of damage at previous times 𝜏 ≤ 𝑡. 
𝑡  is the value of 𝜔𝛼 for the current time (load state), and 𝜔𝛼
𝜏 represents the state 
Damage is applied by scaling the layer stress by reduction parameters 
𝑅𝛼 = 1 − 𝜔𝛼 
where  𝛼 = 𝑓 and  𝛼 = 𝑚.    The  layer  stresses  are  summed  and  then  then  scaled  by 
reduction parameter 
𝑅𝐿 = 1 − 𝜔𝐿. 
Figures  M219-1  (a)  and  (b)  show  the  relationship  between  the  damage  and  reduction 
parameters
If the parameter RESIDS > 0, damage in the layers is limited such that 
𝑅𝑓 = max(RESIDS, 1 − 𝜔𝑓 ) 
𝑅𝑚 = max(RESIDS, 1 − 𝜔𝑚) 
Element Erosion: 
When  ERODE > 0,  an  erosion  criterion  is  checked  at  each  integration  point.    Shell 
elements  and  thick  shell  elements  will  be  deleted  when  the  erosion  criterion  has  been 
met at all integration points.  Brick elements will be deleted when the erosion criterion 
is  met  at  any  of  the  integration  points.    For  ERODE = 1,  the  erosion  criterion  is  met 
when  maximum  principal  strain  exceeds  either  SLOCT ×  ERPAR1  for  elements  in 
tension,  or  SLOCC ×  ERPAR1  for  elements  in  compression.    Elements  are  in  tension 
when  the  magnitude  of  the  first  principal  strain  is  greater  than  the  magnitude  of  the 
third  principal  strain  and  in  compression  when  the  third  principal  strain  is  larger.  
When  𝑅 > 0,  the  ERODE = 1  criterion  is  checked  using  the  non-local  (averaged) 
principal  strain.    For  ERODE = 2,  the  erosion  criterion  is  met  when  the  local  (non-
averaged)  maximum  principal  strain  exceeds  ERPAR2.    For  ERODE = 3,  both  of  these 
erosion  criteria  are  checked.    For  visualization  purposes,  the  ratio  of  the  maximum 
principal strain over the limit is stored in the location of plastic strain which is written 
by default to the elout and d3plot files. 
History Variables: 
History  variables  for  CODAM2  are  enumerated  in  the  following  tables.    To  include 
them in the D3PLOT database, use NEIPH (bricks) or NEIPS (shells) on *DATABASE_-
EXTENT_BINARY.    For  brick  elements,  add  4  to  the  variable  numbers  in  the  table 
because the first 6 history variables are reserved.
*MAT_219 
VARIABLE # 
DESCRIPTION
3 
4 
5 
6 
7 
8 
⋮ 
Overall (anti-locking) Damage. 
Delamination Damage (for visualization only) 
Fiber damage in the first layer 
Matrix damage in the first layer 
Fiber damage in the second layer 
Matrix damage in the second layer 
⋮ 
3 + 2 × NLAYER 
Fiber damage in the last layer 
4 + 2 × NLAYER 
Matrix damage in the last layer 
Equivalent Strains used to evaluate damage (averaged if R1 > 0) 
DESCRIPTION
VARIABLE # 
5 + 2 × NLAYER 
6 + 2 × NLAYER 
7 + 2 × NLAYER 
8 + 2 × NLAYER 
9 + 2 × NLAYER 
⋮ 
4 + 4 × NLAYER 
5 + 4 × NLAYER 
eq 
𝜀𝑅
eq  
𝜀𝑓 ,1
eq  
𝜀𝑚,1
eq  
𝜀𝑓 ,2
eq  
𝜀𝑚,2
  ⋮  
eq  
𝜀𝑓 ,𝑛
eq  
𝜀𝑓 ,𝑛
*MAT_219 
Total Strain 
VARIABLE # 
6 + 4 × NLAYER 
7 + 4 × NLAYER 
8 + 4 × NLAYER 
9 + 4 × NLAYER 
10 + 4 × NLAYER 
11 + 4 × NLAYER 
𝜀𝑥 
𝜀𝑦 
𝜀𝑧 
𝛾𝑥𝑦 
𝛾𝑦𝑧 
𝛾𝑧𝑥
*MAT_220 
This  is  Material  Type  220,  a  rigid  material  for  shells  or  solids.    Unlike  *MAT_020,  a 
*MAT_220  part  can  be    discretized  into  multiple  disjoint  pieces  and  have  each  piece 
behave as an independent rigid body.  The inertia properties for the disjoint pieces are 
determined directly from the finite element discretization.   
Nodes of a *MAT_220 part cannot be shared by any other  rigid part.  A *MAT_220 part 
may share nodes with deformable structural and solid elements.   
This material option can be used to model granular material where the grains interact 
through  an  automatic  single  surface  contact  definition.    Another  possible  use  includes 
modeling bolts as rigid bodies where the bolts belong to the same part ID.  This model 
eliminates the need to represent each rigid piece with a unique part ID. 
5 
6 
7 
8 
Card 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
Default 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio.
*MAT_ORTHOTROPIC_SIMPLIFIED_DAMAGE 
This  is  Material  Type  221.    An  orthotropic  material  with  optional  simplified  damage 
and  optional  failure  for  composites  can  be  defined.    This  model  is  valid  only  for  3D 
solid  elements,  with  reduced  or  full  integration.    The  elastic  behavior  is  the  same  as 
MAT_022.  Nine damage variables are defined such that damage is different in tension 
and compression.  These damage variables are applicable to 𝐸𝑎, 𝐸𝑏, 𝐸𝑐, 𝐺𝑎𝑏, 𝐺𝑏𝑐 and 𝐺𝑐𝑎.  
In addition, nine failure criteria on strains are available.  When failure occurs, elements 
are  deleted  (erosion).    Failure  depends  on  the  number  of  integration  points  failed 
through the element.  See the material description below. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
EA 
F 
4 
EB 
F 
5 
EC 
F 
6 
7 
8 
PRBA 
PRCA 
PRCB 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
GAB 
GBC 
GCA 
AOPT 
MACF 
Type 
F 
F 
F 
Default 
none 
none 
none 
  Card 3 
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
3 
ZP 
F 
4 
A1 
F 
F 
0.0 
5 
A2 
F 
I 
0 
6 
A3 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
7
Card 4 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
7 
8 
BETA 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NERODE 
NDAM 
EPS1TF 
EPS2TF 
EPS3TF 
EPS1CF 
EPS2CF 
EPS3CF 
Type 
Default 
I 
0 
  Card 6 
1 
I 
0 
2 
F 
F 
F 
F 
F 
F 
1020 
1020 
1020 
-1020 
-1020 
-1020 
3 
4 
5 
6 
7 
8 
Variable 
EPS12F 
EPS23F 
EPS13F 
EPSD1T 
EPSC1T  CDAM1T 
EPSD2T 
EPSC2T 
Type 
F 
F 
F 
Default 
1020 
1020 
1020 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
  Card 7 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CDAM2T 
EPSD3T 
EPSC3T  CDAM3T 
EPSD1C 
EPSC1C  CDAM1C  EPSD2C 
Type 
I 
Default 
0. 
I 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0.
Card 8 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EPSC2C  CDAM2C  EPSD3C 
EPSC3C  CDAM3C 
EPSD12 
EPSC12  CDAM12 
Type 
F 
Default 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
  Card 9 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EPSD23 
EPSC23  CDAM23 
EPSD31 
EPSC31  CDAM31 
Type 
F 
Default 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
  VARIABLE   
DESCRIPTION
MID 
RO 
EA 
EB 
EC 
PRBA 
PRCA 
PRCB 
GAB 
GBC 
GCA 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
𝐸𝑎, Young’s modulus in 𝑎-direction 
𝐸𝑏, Young’s modulus in 𝑏-direction 
𝐸𝑐, Young’s modulus in 𝑐-direction 
𝜈𝑏𝑎, Poisson ratio 
𝜈𝑐𝑎, Poisson ratio 
𝜈𝑐𝑏, Poisson ratio 
𝐺𝑎𝑏, Shear modulus 
𝐺𝑏𝑐, Shear modulu 
𝐺𝑐𝑎, Shear modulus
VARIABLE   
AOPT 
DESCRIPTION
Material  axes  option  : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element  nodes  1,  2,  and  4,  as  with  *DEFINE_
COORDINATE_NODES. 
EQ.1.0: locally orthotropic with material axes determined by a
point  in  space  and  the  global  location  of  the  element
center;  this  is  the  𝑎-direction.    This  option  is  for  solid 
elements only. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
*DEFINE_
as  with 
below, 
vectors 
COORDINATE_VECTOR. 
defined 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  𝐯  with  the 
element normal. 
EQ.4.0: locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector  𝐯,  and 
an originating point, 𝐩, which define the centerline ax-
is.  This option is for solid elements only. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_
*DEFINE_COORDINATE_SYSTEM 
COORDINATE_VECTOR). 
or 
MACF 
Material axes change flag for brick elements: 
EQ.1: No change, default, 
EQ.2: switch material axes 𝐚 and 𝐛, 
EQ.3: switch material axes 𝐚 and 𝐜, 
EQ.4: switch material axes 𝐛 and 𝐜. 
XP, YP, ZP 
Coordinates of point 𝐩 for AOPT = 1 and 4 
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3 and 4 
D1, D2, D3 
Components of vector 𝐝 for AOPT = 2
BETA 
NERODE 
*MAT_ORTHOTROPIC_SIMPLIFIED_DAMAGE 
DESCRIPTION
Material  angle  in  degrees  for  AOPT = 3,  may  be  overridden  on 
the element card, see  *ELEMENT_SOLID_ORTHO. 
Element  erosion  flag.   For  multi-integration point  elements,  each 
of the failure strains mentioned below for NERODE 2 and higher 
need  only  occur  in  one  integration  point  to  trigger  element
erosion,  and  for  NERODE  values  6  to  11,    which  require  more
than  one  failure  strain  be  reached,  those  failure  strains  need  not
occur in the same integration point.   
EQ.0: No erosion (default). 
EQ.1: Erosion  occurs  when  one  failure  strain  is  reached  in  all 
integration points.  
EQ.2: Erosion occurs when one failure strain is reached.  
EQ.3: Erosion  occurs  when  a  tension  or  compression  failure 
strain in the 𝑎-direction is reached. 
EQ.4: Erosion occurs when as a tension or compression failure 
strain in the 𝑏-direction is reached. 
EQ.5: Erosion  occurs  when  a  tension  or  compression  failure 
strain in the 𝑐-direction is reached. 
EQ.6: Erosion  occurs  when  tension  or  compression  failure 
strain in both the 𝑎- and 𝑏-directions are reached. 
EQ.7: Erosion  occurs  when  tension  or  compression  failure 
strain in both the 𝑏- and 𝑐-directions are reached. 
EQ.8: Erosion  occurs  when  tension  or  compression  failure 
strain in both the 𝑎- and 𝑐-directions are reached. 
EQ.9: Erosion  occurs  when  tension  or  compression  failure 
strain in all 3 directions are reached.  
EQ.10:Erosion  occurs  when  tension  or  compression  failure 
strain  in  both  the  𝑎-  and  𝑏-directions  are  reached  and 
either of the out-of-plane failure shear strains (bc or ac) is 
reached.  .  
EQ.11:Erosion occurs when tension failure strain in either the 𝑎-
or  𝑏-directions  is  reached  and  either  of  the  out-of-plane
failure shear strains (bc or ac) is reached.
VARIABLE   
DESCRIPTION
NDAM 
Damage flag: 
EQ.0: No damage (default) 
EQ.1: Damage in tension only (null for compression) 
EQ.2: Damage in tension and compression 
EPS1TF 
Failure strain in tension along the 𝑎-direction 
EPS2TF 
Failure strain in tension along the 𝑏-direction 
EPS3TF 
Failure strain in tension along the 𝑐-direction 
EPS1CF 
Failure strain in compression along the 𝑎-direction 
EPS2CF 
Failure strain in compression along the 𝑏-direction 
EPS3CF 
Failure strain in compression along the 𝑐-direction 
EPS12F 
Failure shear strain in the 𝑎𝑏-plane 
EPS23F 
Failure shear strain in the 𝑏𝑐-plane 
EPS13F 
Failure shear strain in the 𝑎𝑐-plane 
EPSD1T 
EPSC1T 
𝑠  
Damage threshold in tension along the 𝑎-direction, 𝜀1𝑡
𝑐  
Critical damage threshold in tension along the 𝑎-direction, 𝜀1𝑡
CDAM1T 
𝑐  
Critical damage in tension along the 𝑎-direction, 𝐷1𝑡
EPSD2T 
EPSC2T 
𝑠  
Damage threshold in tension along the 𝑏-direction, 𝜀2𝑡
𝑐  
Critical damage threshold in tension along the b-direction, 𝜀2𝑡
CDAM2T 
𝑐  
Critical damage in tension along the 𝑏-direction, 𝐷2𝑡
EPSD3T 
EPSC3T 
𝑠  
Damage threshold in tension along the 𝑐-direction, 𝜀3𝑡
𝑐  
Critical damage threshold in tension along the 𝑐-direction, 𝜀3𝑡
CDAM3T 
𝑐  
Critical damage in tension along the 𝑐-direction, 𝐷3𝑡
EPSD1C 
EPSC1C 
𝑠  
Damage threshold in compression along the 𝑎-direction, 𝜀1𝑐
Critical  damage  threshold  in  compression  along  the  𝑎-direction, 
𝑐  
𝜀1𝑐
*MAT_ORTHOTROPIC_SIMPLIFIED_DAMAGE 
DESCRIPTION
CDAM1C 
𝑐  
Critical damage in compression along the 𝑎-direction, 𝐷1𝑐
EPSD2C 
EPSC2C 
𝑠  
Damage threshold in compression along the 𝑏-direction, 𝜀2𝑐
Critical  damage 
𝑐  
direction, 𝜀2𝑐
threshold 
in  compression  along 
the  𝑏-
CDAM2C 
𝑐  
Critical damage in compression along the 𝑏-direction, 𝐷2𝑐
EPSD3C 
EPSC3C 
𝑠  
Damage threshold in compression along the 𝑐-direction, 𝜀3𝑐
Critical  damage  threshold  in  compression  along  the  𝑐-direction, 
𝑐  
𝜀3𝑐
CDAM3C 
𝑐  
Critical damage in compression along the 𝑐-direction, 𝐷3𝑐
EPSD12 
EPSC12 
𝑠  
Damage threshold for shear in the 𝑎𝑏-plane, 𝜀12
𝑐  
Critical damage threshold for shear in the 𝑎𝑏-plane, 𝜀12
CDAM12 
𝑐  
Critical damage for shear in the 𝑎𝑏-plane, 𝐷12
EPSD23 
EPSC23 
𝑠  
Damage threshold for shear in the 𝑏𝑐-plane, 𝜀23
𝑐  
Critical damage threshold for shear in the 𝑏𝑐-plane, 𝜀23
CDAM23 
𝑐  
Critical damage for shear in the 𝑏𝑐-plane, 𝐷23
EPSD31 
EPSC31 
𝑠  
Damage threshold for shear in the 𝑎𝑐-plane, 𝜀31
𝑐  
Critical damage threshold for shear in the 𝑎𝑐-plane, 𝜀31
CDAM31 
𝑐  
Critical damage for shear in the 𝑎𝑐-plane, 𝐷31
Remarks: 
If 𝜀𝑘
𝑐 < 𝜀𝑘
𝑠  , no damage is considered.  Failure occurs only when failure strain is reached. 
Failure can occur along the 3 orthotropic directions, in tension, in compression and for 
shear behavior.  Nine failure strains drive the failure.  When failure occurs, elements are 
deleted  (erosion).    Under  the  control  of  the  NERODE  flag,  failure  may  occur  either 
when only one integration point has failed, when several integration points have failed 
or when all integrations points have failed.
Damage applies to the 3 Young’s moduli and the 3 shear moduli.  Damage is different 
for tension and compression.  Nine damage variables are used: 𝑑1𝑡, 𝑑2𝑡, 𝑑3𝑡, 𝑑1𝑐, 𝑑2𝑐, 𝑑3𝑐, 
𝑑12, 𝑑23, 𝑑13.  The damaged flexibility matrix is: 
𝐸𝑎(1 − 𝑑1[𝑡,𝑐])
−𝜐𝑏𝑎
𝐸𝑏
−𝜐𝑐𝑎
𝐸𝑐
−𝜐𝑏𝑎
𝐸𝑏
𝐸𝑏(1 − 𝑑2[𝑡,𝑐])
−𝜐𝑐𝑏
𝐸𝑐
−𝜐𝑐𝑎
𝐸𝑐
−𝜐𝑐𝑏
𝐸𝑐
𝐸𝑐(1 − 𝑑3[𝑡,𝑐])
𝐺𝑎𝑏(1 − 𝑑12)
𝐺𝑏𝑐(1 − 𝑑23)
 𝑆dam =
⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛
⎝
The nine damage variables are calculated as follows: 
𝑑𝑘 = max (𝑑𝑘; 𝐷𝑘
𝑐 ⟨
𝜀𝑘 − 𝜀𝑘
𝑠 ⟩
𝑐 − 𝜀𝑘
𝜀𝑘
+
) 
⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞
𝐺𝑐𝑎(1 − 𝑑31)⎠
with k = 1t, 2t, 3t, 1c, 2c, 3c, 12, 23, 31. 
⟨
⟩+ is the positive part: ⟨𝑥⟩+ = {
if  x > 0
if  x < 0
. 
Damage in compression may be deactivated with the NDAM flag.  In this case, damage 
in  compression  is  null,  and  only  damage  in  tension  and  for  shear  behavior  are  taken 
into account. 
The  nine  damage  variables  may  be  post-processed  through  additional  variables.    The 
number of additional variables for solids written to the d3plot and d3thdt databases is 
input by the optional *DATABASE_EXTENT_BINARY card as variable NEIPH.  These 
additional variables are tabulated below: 
History 
Variable 
Description 
Value 
𝑑1𝑡 
𝑑2𝑡 
𝑑3𝑡 
𝑑1𝑐 
𝑑2𝑐 
𝑑3𝑐 
𝑑12 
damage in traction along 𝑎 
damage in traction along 𝑏 
damage in traction along 𝑐 
damage in compression along 𝑎 
0 - no damage 
damage in compression along 𝑏 
damage in compression along 𝑐 
0 < 𝑑𝑘 < 𝐷𝑘
𝑐 - damage 
shear damage in 𝑎𝑏-plane 
LS-PrePost 
History Variable
plastic strain 
1 
2 
3 
4 
5
History 
Variable 
Description 
Value 
𝑑23 
𝑑13 
shear damage in 𝑏𝑐-plane 
shear damage in 𝑎𝑐-plane 
LS-PrePost 
History Variable
7 
8 
The first damage variable is stored as in the place of effective plastic strain.  The eight 
other damage variables may be plotted in LS-PrePost as element history variables.
*MAT_TABULATED_JOHNSON_COOK 
This  is Material  Type  224.    An  elasto-viscoplastic  material  with  arbitrary  stress  versus 
strain  curve(s)  and  arbitrary  strain  rate  dependency  can  be  defined.    Plastic  heating 
causes  adiabatic  temperature  increase  and  material  softening.    Optional  plastic  failure 
strain can be defined as a function of triaxiality, strain rate, temperature and/or element 
size.    Please  take  careful  note  the  sign  convention  of  triaxiality  used  for  *MAT_224  as 
illustrated in Figure M224-1.  
This material model resembles the original Johnson-Cook material  but 
with the possibility of general tabulated input parameters. 
An equation of state (*EOS) is optional for solid elements, tshell formulations 3 and 5, 
and  2D  continuum  elements,  and  is  invoked  by  setting  EOSID  to  a  nonzero  value  in 
*PART.  If an equation of state is used, only the deviatoric stresses are calculated by the 
material model and the pressure is calculated by the equation of state. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
CP 
F 
6 
TR 
F 
7 
8 
BETA 
NUMINT 
F 
F 
Default 
none 
none 
none 
none 
none 
0.0 
1.0 
1.0 
  Card 2 
1 
2 
3 
4 
5 
Variable 
LCK1 
LCKT 
LCF 
LCG 
LCH 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
6 
LCI 
F 
0 
7
*MAT_TABULATED_JOHNSON_COOK 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FAILOPT  NUMAVG  NCYFAIL 
ERODE 
LCPS 
Type 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
CP 
TR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus: 
GT.0.0: constant value is used 
LT.0.0:  -E gives curve ID for temperature dependence  
Poisson’s ratio. 
Specific heat (superseded by heat capacity in *MAT_THERMAL_
OPTION if a coupled thermal/structural analysis). 
Room temperature. 
BETA 
Fraction of plastic work converted into heat: 
GT.0.0: constant value is used 
LT.0.0:  -BETA  gives  either  a  curve  ID  for  strain  rate
dependence  or  a  table  ID  for  strain  rate  and  tempera-
ture dependence.
VARIABLE   
NUMINT 
DESCRIPTION
GT.0.0:  Number of integration points which must fail before
the  element  is  deleted.    Available  for  shells  and  sol-
ids. 
LT.0.0: 
-NUMINT  is  percentage  of  integration  points/layers
which  must  fail  before  shell  element  fails.    For  fully
integrated shells, a methodology is used where a lay-
er fails if one integration point fails and then the giv-
en  percentage  of  layers  must  fail  before  the  element
fails.  Only available for shells except as noted below
EQ.-200:  Turns  off  erosion  for  shells  and  solids. 
recommended  unless  used 
*CONSTRAINED_TIED_NODES_FAILURE. 
  Not
in  conjunction  with
LCK1 
LCKT 
LCF 
LCG 
LCH 
Load  curve  ID  or  Table  ID.    The  load  curve  ID  defines  effective
stress as a function of effective plastic strain.  The table ID defines
for  each  plastic  strain  rate  value  a  load  curve  ID  giving  the
(isothermal) effective stress versus effective plastic strain for that 
rate.    As  in  *MAT_024,  natural  logarithmic  strain  rates  can  be 
used by setting the first strain rate to a negative value. 
Table  ID  defining  for  each  temperature  value  a  load  curve  ID
giving  the  (quasi-static)  effective  stress  versus  effective  plastic 
strain for that temperature. 
Load  curve  ID  or  Table  ID.    The  load  curve  ID  defines  plastic
failure  strain  (or  scale  factor  –  see  Remarks)  as  a  function  of 
triaxiality.    The  table  ID  defines  for  each  Lode  parameter  a  load 
curve ID giving the plastic failure strain versus triaxiality for that
Lode  parameter.    (Table  option  only  for  solids  and  not  yet
generally  supported).    See  Remarks  for  a  description  of  the
combination of LCF, LCG, LCH, and LCI. 
Load curve ID defining plastic failure strain (or scale factor – see 
Remarks)  as  a  function  of  plastic  strain  rate.    If  the  first  abscissa 
value  in  the  curve  corresponds  to  a  negative  strain  rate,  LS-
DYNA assumes that the natural logarithm of the strain rate value
is  used  for  all  abscissa  values.    See  Remarks  for  a  description  of
the combination of LCF, LCG, LCH, and LCI. 
Load curve ID defining plastic failure strain (or scale factor – see 
Remarks)  as  a  function  of  temperature.    See  Remarks  for  a
description of the combination of LCF, LCG, LCH, and LCI.
LCI 
*MAT_TABULATED_JOHNSON_COOK 
DESCRIPTION
Load  curve  ID,  Table  ID,  or  Table_3D  ID.    The  load  curve  ID
defines  plastic  failure  strain  (or  scale  factor  –  see  Remarks)  as  a 
function of element size.  The table ID defines for each triaxiality a
load curve ID giving the plastic failure strain versus element size
for  that  triaxiality.    If  a  three  dimensional  table  ID  is  referred,
plastic  failure  strain  can  be  a  function  of  Lode  parameter
(TABLE_3D), triaxiality (TABLE), and element size (CURVE).  See
Remarks for a description of the combination of LCF, LCG, LCH,
and LCI. 
FAILOPT 
Flag for additional failure criterion 𝐹2, see Remarks. 
EQ.0.0: off (default) 
EQ.1.0: on 
NUMAVG 
NCYFAIL 
Number of time steps for running average of plastic failure strain
in the additional failure criterion.  Default is 1 (no averaging). 
Number of time steps that the additional failure criterion must be
met before element deletion.  Default is 1. 
ERODE 
Erosion flag (only for solid elements):  
EQ.0.0: default, element erosion is allowed. 
EQ.1.0: element  does  not  erode;  deviatoric  stresses  set  to  zero
when element fails. 
Table  ID  with  first  principal  stress  limit  as  function  of  plastic
strain  (curves)  and  plastic  strain  rate  (table).    This  option  is  for
post-processing purposes only and gives an indication of areas in
the structure where failure is likely to occur.  History variable #17 
shows a value of 1.0 for integration points that exceeded the limit,
else a value of 0.0. 
LCPS 
Remarks: 
The flow stress 𝜎𝑦 is expressed as a function of plastic strain 𝜀𝑝, plastic strain rate 𝜀̇𝑝 and 
temperature 𝑇 via the following formula (using load curves/tables LCK1 and LCKT):
𝑠𝑦 = 𝑘1(𝜀𝑝, 𝜀̇𝑝)
𝑘𝑡(𝜀𝑝, 𝑇)
𝑘𝑡(𝜀𝑝, 𝑇𝑅)
Note  that  𝑇𝑅  is  a  material  parameter  and  should  correspond  to  the  temperature  used 
when performing the room temperature tensile tests.  If simulations are to be performed
plastic
failure
strain
tension
compression
-2/3
-1/3
triaxiality
p/σ
vm
1/3
2/3
Figure  M224-1.    Typical  failure  curve  for  metal  sheet,  modeled  with  shell
elements. 
with  an  initial  temperature  TI  deviating  from  𝑇𝑅  then  this  temperature  should  be  set 
using  *INITIAL_STRESS_SOLID/SHELL  by  setting  history  variable  #14  for  solid 
elements or history variable #10 for shell elements. 
Optional  plastic  failure  strain  is  defined  as  a  function  of  triaxiality
parameter, plastic strain rate
element area for shells and volume over maximum area for solids) by 
𝑝/𝜎𝑣𝑚,  Lode 
𝜀̇𝑝, temperature 𝑇 and initial element size 𝑙c (square root of 
𝜀𝑝𝑓 = 𝑓 (
𝜎vm
,
27𝐽3
2𝜎vm
3 ) 𝑔(𝜀̇𝑝)ℎ(𝑇)𝑖 (𝑙𝑐,
𝜎vm
) 
using  load  curves/tables  LCF,  LCG,  LCH  and  LCI.    If  more  than  one  of  these  four 
variables  LCF,  LCG,  LCH  and  LCI  are  defined,  be  aware  that  the  net  plastic  failure 
strain  is  essentially  the  product of  multiple  functions  as  shown  in  the  above  equation.  
This means that one and only one of the variables LCF, LCG, LCH, and LCI can point to 
curve(s)  that  have  plastic  strain  along  the  curve  ordinate.    The  remaining  nonzero 
variable(s)  LCF,  LCG,  LCH,  and  LCI    should  point  to  curve(s)  that  have  a  unitless 
scaling factor along the curve ordinate.   
A  typical  failure  curve  LCF  for  metal  sheet,  modeled  with  shell  elements  is  shown  in 
Figure  M224-1.    Triaxiality  should  be  monotonically  increasing  in  this  curve.    A 
reasonable  range  for  triaxiality  is  -2/3  to  2/3  if  shell  elements  are  used  (plane  stress).  
For  3-dimensional  stress  states  (solid  elements),  the  possible  range  of  triaxiality  goes 
from  -∞  to  +∞,  but  to  get  a  good  resolution  in  the  internal  load  curve  discretization 
(depending on parameter LCINT of *CONTROL_SOLUTION) one should define lower 
limits, e.g.  -1 to 1 if LCINT = 100 (default).  
The default failure criterion of this material model depends on plastic strain evolution 
𝜀̇𝑝 and on plastic failure strain 𝜀𝑝𝑓  and is obtained by accumulation over time:
𝐹 = ∫
𝜀̇𝑝
𝜀𝑝𝑓
𝑑𝑡 
where  element  erosion  takes  place  when  𝐹 ≥ 1.  This  accumulation  provides  load-path 
dependent treatment of failure.  The value of 𝐹  is stored as history variable #8 for shells 
and #12 for solids.   
An  additional,  load-path  independent,  failure  criterion  can  be  invoked  by  setting 
FAILOPT = 1, where the current state of plastic strain is used: 
𝐹2 =
𝜀𝑝
𝜀𝑝𝑓
Two  additional  parameters  can  be  used  as  countermeasures  against  stress  oscillations 
for this failure criterion.  With NUMAVG active, plastic failure strain is averaged over 
NUMAVG  time  steps  for  the  𝐹2  criterion.    The  value  of  𝐹2,  taking  into  account  any 
averaging  per NUMAVG, is stored as history variable #14 for shells and #16 for solids.  
NUMAVG  cannot  exceed  30.    NCYFAIL  defines  the  number  of  time  steps  that  𝐹2 ≥ 1 
must be met before element deletion takes place.  The number of time steps that 𝐹2 ≥ 1 
is stored as history variable #15 for shells and #19 for solids. 
Temperature increase is caused by plastic work 
𝑇 = 𝑇𝑅 +
𝐶𝑝𝜌
∫ 𝜎𝑦𝜀̇𝑝𝑑𝑡 
with room temperature 𝑇𝑅, dissipation factor 𝛽, specific heat 𝐶𝑝, and density 𝜌. 
For  *CONSTRAINED_TIED_NODES_WITH_FAILURE,  the  failure  is  based  on  the 
damage instead to the plastic strain. 
History variables may be post-processed through additional variables.  The number of 
additional variables for shells/solids written to the d3plot and d3thdt databases is input 
by the optional *DATABASE_EXTENT_BINARY card as variable NEIPS/NEIPH.  The 
relevant additional variables of this material model are tabulated below:
LS-PrePost  
history 
variable # 
1 
7 
8 
9 
10 
11 
12 
17 
Shell elements 
plastic strain rate 
plastic work 
ratio of plastic strain to 
plastic failure strain 
element size 
temperature 
plastic failure strain 
triaxiality 
LCPS: critical value  
LS-PrePost  
history 
variable # 
5 
8 
9 
10 
11 
12 
13 
14 
17 
Solid elements 
plastic strain rate 
plastic failure strain 
triaxiality 
Lode parameter 
plastic work 
ratio of plastic strain to 
plastic failure strain 
element size 
temperature 
LCPS: critical value
*MAT_TABULATED_JOHNSON_COOK_GYS 
This is Material Type 224_GYS.  This is an isotropic elastic plastic material law with J3 
dependent yield surface.  This material considers tensile/compressive asymmetry in the 
material  response,  which  is  important  for  HCP  metals  like  Titanium.    The  model  is 
available for solid elements. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
CP 
F 
6 
TR 
F 
7 
8 
BETA 
NUMINT 
F 
F 
Default 
none 
none 
none 
none 
none 
0.0 
1.0 
1.0 
  Card 2 
1 
2 
3 
4 
5 
Variable 
LCK1 
LCKT 
LCF 
LCG 
LCH 
Type 
Default 
F 
0 
  Card 3 
1 
F 
0 
2 
F 
0 
3 
F 
0 
4 
F 
0 
5 
6 
LCI 
F 
0 
6 
7 
8 
7 
8 
Variable 
LCCR 
LCCT 
LCSR 
LCST 
IFLAG 
SFIEPM 
NITER 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
1 
100 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density.
VARIABLE   
DESCRIPTION
E 
Young’s modulus: 
GT.0.0: constant value is used 
LT.0.0:  temperature  dependent  Young’s  modulus  given  by
load curve ID = -E 
PR 
CP 
TR 
Poisson’s ratio. 
Specific heat. 
Room temperature. 
BETA 
Fraction of plastic work converted into heat. 
NUMINT 
Number of integration points which must fail before the element
is deleted. 
LCK1 
LCKT 
LCF 
LCG 
LCH 
LCI 
EQ.-200:  Turns  off  erosion  for  solids.    Not  recommended
unless  used  in  conjunction  with  *CONSTRAINED_-
TIED_NODES_FAILURE. 
Table ID defining for each plastic strain rate value a load curve ID 
giving  the  (isothermal)  effective  stress  versus  effective  plastic
strain for that rate. 
Table  ID  defining  for  each  temperature  value  a  load  curve  ID
giving  the  (quasi-static)  effective  stress  versus  effective  plastic
strain for that temperature. 
Load  curve  ID  or  Table  ID.    The  load  curve  ID  defines  plastic
failure strain as a function of triaxiality.  The table ID defines for
each  Lode  parameter  a  load  curve  ID  giving  the  plastic  failure
strain  versus  triaxiality  for  that  Lode  parameter.    (Table  option 
only for solids and not yet generally supported). 
Load  curve  ID  defining  plastic  failure  strain  as  a  function  of
plastic strain rate. 
Load  curve  ID  defining  plastic  failure  strain  as  a  function  of
temperature 
Load  curve  ID  or  Table  ID.    The  load  curve  ID  defines  plastic
failure  strain  as  a  function  of  element  size.    The  table  ID  defines
for each triaxiality a load curve ID giving the plastic failure strain
versus element size for that triaxiality.
VARIABLE   
LCCR 
LCCT 
LCSR 
LCST 
DESCRIPTION
Table ID.  The curves in this table define compressive yield stress
as  a  function  of  plastic  strain  or  effective  plastic  strain  .  The table ID defines for each plastic strain rate value or
effective  plastic  strain  rate  value  a  load  curve  ID  giving  the 
(isothermal)  compressive  yield  stress  versus  plastic  strain  or
effective plastic strain for that rate. 
Table  ID  defining  for  each  temperature  value  a  load  curve  ID
giving the (quasi-static) compressive yield stress versus strain for
that  temperature.    The  curves  in  this  table  define  compressive
yield stress as a function of plastic strain or effective plastic strain
. 
Table ID.  The load curves define shear yield stress in function of
plastic  strain  or  effective  plastic  strain  .The  table  ID 
defines for each plastic strain rate value or effective plastic strain
rate  value  a  load  curve  ID  giving  the  (isothermal)  shear  yield
stress versus plastic strain or effective plastic strain for that rate. 
Table  ID  defining  for  each  temperature  value  a  load  curve  ID
giving  the  (quasi-static)  shear  yield  stress  versus  strain  for  that
temperature.    The  load  curves  define  shear  yield  stress  as  a
function of plastic strain or effective plastic strain . 
IFLAG 
Flag to specify abscissa for LCCR, LCCT, LCSR, LCST: 
EQ.0.0: Compressive and shear yields are given in a function of
plastic strain as defined in the remarks (default). 
EQ.1.0: Compressive and shear yields are given in function of
effective plastic strain. 
SFIEPM 
Scale factor on the initial estimate of the plastic multiplier. 
NITER 
Number of secant iterations to be performed. 
Remarks: 
If IFLAG = 0 the compressive and shear curves are defined as follows: 
σ𝑐(𝜀𝑝𝑐, 𝜀̇𝑝𝑐),     𝜀𝑝𝑐 = 𝜀𝑐 −
σ𝑠(𝛾𝑝𝑠, 𝛾̇𝑝𝑠),     𝛾𝑝𝑠 = 𝛾𝑠 −
𝜎𝑐
𝜎𝑠
,     𝜀̇𝑝𝑐 =  
,     𝛾̇𝑝𝑠 =  
𝜕𝜀𝑝𝑐
𝜕𝑡
𝜕𝛾𝑝𝑠
𝜕𝑡
and two new history variables (#16 plastic strain in compression and #17 plastic strain 
in shear)  are stored in addition to those history variables already stored in MAT_224. 
If IFLAG = 1 the compressive and shear curves are defined as follows: 
σ𝑐(𝜆̇, 𝜆),     𝜎𝑠(𝜆̇, 𝜆),     𝑊𝑝̇ = 𝜎eff𝜆̇ 
History variables may be post-processed through additional variables.  The number of 
additional variables for solids written to the d3plot and d3thdt databases is input by the 
optional  *DATABASE_EXTENT_BINARY  card  as  variable  NEIPH.    The  relevant 
additional variables of this material model are tabulated below: 
LS-PrePost  history 
variable # 
5 
8 
9 
10 
11 
12 
13 
14 
16 
17 
Solid elements 
plastic strain rate 
plastic failure strain 
triaxiality 
Lode parameter 
plastic work 
damage 
element size 
temperature 
plastic strain in compression 
plastic strain in shear
*MAT_VISCOPLASTIC_MIXED_HARDENING 
This is Material Type 225.  An elasto-viscoplastic material with an arbitrary stress versus 
strain curve and arbitrary strain rate dependency can be defined.  Kinematic, isotropic, or a 
combination of kinematic and isotropic hardening can be specified.  Also, failure based on 
plastic strain can be defined. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
6 
7 
8 
LCSS 
BETA 
I 
F 
Default 
none 
none 
none 
none 
none 
0.0 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FAIL 
Type 
F 
Default  1.0E+20 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio.
VARIABLE   
LCSS 
DESCRIPTION
Load  curve  ID  or  Table  ID.    Load  curve  ID  defining  effective
stress versus effective plastic strain The table ID defines for each
strain rate value a load curve ID giving the stress versus effective
plastic  strain  for  that  rate,  See  Figure  M24-1.    The  stress  versus 
effective  plastic  strain  curve  for the  lowest  value  of  strain  rate  is
used if the strain rate falls below the minimum value.  Likewise,
the stress versus effective plastic strain curve for the highest value 
of strain rate is used if the strain rate exceeds the maximum value.
NOTE: The strain rate values defined in the table may be given as
the  natural  logarithm  of  the  strain  rate.    If  the  first  stress-strain 
curve in the table corresponds to a negative strain rate, LS-DYNA 
assumes that the natural logarithm of the strain rate value is used.
Since  the  tables  are  internally  discretized  to  equally  space  the
points,  natural  logarithms  are  necessary,  for  example,  if  the
curves  correspond to rates from 10.e-04 to 10.e+04. 
BETA 
Hardening parameter, 0 < BETA < 1. 
EQ.0.0: 
EQ.1.0: 
Pure kinematic hardening 
Pure isotropic hardening 
0.0 < BETA < 1.0:  Mixed hardening 
FAIL 
Failure flag. 
LT.0.0:  User  defined  failure  subroutine  is  called  to  determine
failure 
EQ.0.0: Failure is not considered.  This option is recommended
if  failure is not of interest since many calculations will
be saved. 
GT.0.0:  Plastic  strain  to  failure.    When  the  plastic  strain
reachesthis  value,  the  element  is  deleted  from  the  cal-
culation..
*MAT_KINEMATIC_HARDENING_BARLAT89_{OPTION} 
This  is  Material  Type  226.    This  model  combines  Yoshida  non-linear  kinematic 
hardening  rule  (*MAT_125)  with  the  3-parameter  material  model  of  Barlat  and  Lian 
[1989]  (*MAT_36)  to  model  metal  sheets  under  cyclic  plasticity  loading  and  with 
anisotropy in plane stress condition.  Lankford parameters are used for the definition of 
the  anisotropy.    Yoshida’s  theory  describes  the  hardening  rule  with  ‘two  surfaces’ 
method: the yield surface and the bounding surface.  In the forming process, the yield 
surface  does  not  change  in  size,  but  its  center  moves  with  deformation;  the  bounding 
surface changes both in size and location. 
Available options include: 
<BLANK> 
NLP 
The NLP option estimates failure using the Formability Index (F.I.), which accounts for 
the non-linear strain paths seen in metal forming applications .  When the 
NLP  option  is  invoked,  the  variable  IFLD must  be  specified.    Additionally,  the  option 
NLP is also available in *MAT_036, *MAT_037 and *MAT_125. 
  Card 1 
1 
Variable 
MID 
Type 
I 
2 
RO 
F 
3 
E 
F 
4 
PR 
F 
5 
M 
F 
6 
7 
8 
R00 
R45 
R90 
F 
F 
F 
Default 
none 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
none 
  Card 2 
Variable 
1 
CB 
Type 
F 
2 
Y 
F 
3 
SC 
F 
4 
K 
F 
5 
RSAT 
F 
6 
SB 
F 
7 
H 
F 
8 
HLCID 
I 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
none
Card 3 
1 
2 
Variable 
AOPT 
IOPT 
Type 
F 
I 
3 
C1 
F 
4 
C2 
F 
5 
6 
7 
8 
IFLD 
I 
Default 
none 
none 
0.0 
0.0 
none 
  Card 4 
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
3 
ZP 
F 
4 
A1 
F 
5 
A2 
F 
6 
A3 
F 
7 
8 
Default 
none 
none 
none 
none 
none 
none 
  Card 5 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
7 
8 
BETA 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
MID 
Material identification.  A unique number must be specified. 
RO 
E 
PR 
M 
R00 
R45 
Mass density. 
Young’s modulus, E. 
Poisson’s ratio, ν. 
m, the exponent in Barlat’s yield criterion. 
𝑅00, Lankford parameter in 0 degree direction. 
𝑅45, Lankford parameter in 45 degree direction.
R90 
CB 
Y 
SC 
K 
*MAT_KINEMATIC_HARDENING_BARLAT89 
DESCRIPTION
𝑅90, Lankford parameter in 90 degree direction. 
The uppercase 𝐵 defined in the Yoshida’s equations. 
Hardening parameter as defined in the Yoshida’s equations. 
The lowercase 𝑐 defined in the Yoshida’s equations. 
Hardening parameter as defined in the Yoshida’s equations. 
RSAT 
Hardening parameter as defined in the Yoshida’s equations. 
SB 
H 
HLCID 
The lowercase 𝑏 as defined in the Yoshida’s equations. 
Anisotropic  parameter 
stagnation, defined in the Yoshida’s equations. 
associated  with  work-hardening 
Load  curve  ID  in  keyword  *DEFINE_CURVE,  where  true  strain 
and  true  stress  relationship  is  characterized.    The  load  curve  is
optional, and is used for error calculation only. 
IOPT 
Kinematic hardening rule flag:  
EQ.0: Original Yoshida formulation, 
EQ.1: Modified formulation: define C1, C2 as below. 
C1, C2 
Constants used to modify 𝑅: 
𝑅 = RSAT × [(𝐶1 + 𝜀̅𝑝)𝑐2 − 𝐶1
𝑐2] 
IFLD 
ID  of  a  load  curve  of  the  traditional  Forming  Limit  Diagram
(FLD)  for  the  linear  strain  paths.    In  the  load  curve,  abscissas
represent  minor  strains  while  ordinates  represent  major  strains.
Define only when the NLP option is used.  See the example in the 
remarks section. 
AOPT 
Material axes option : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES,  and  then  rotated  about  the  shell  ele-
ment normal by theangle BETA. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
VARIABLE   
DESCRIPTION
NATE_VECTOR: 
EQ.3.0: locally  orthotropic  material  axes  determined  by 
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the
element normal: 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE__CO-
ORDINATE_VECTOR):Available  with  the  R3  release 
of Version 971 and later. 
XP, YP, ZP 
Coordinates of point 𝐩 for AOPT = 1. 
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3. 
D1, D2, D3 
Components of vector 𝐝 for AOPT = 2. 
BETA 
Material angle in degrees for AOPT = 0 and 3, may be overridden 
on the element card, see *ELEMENT_SHELL_BETA. 
On Barlat and Lian’s yield criteron: 
The  𝑅-values  are  defined  as  the  ratio  of  instantaneous  width  change  to  instantaneous 
thickness  change.    That  is,  assume  that  the  width  𝑊  and  thickness  𝑇  are  measured  as 
function of strain.  Then the corresponding 𝑅-value is given by: 
𝑅 =
𝑑𝑊
𝑑𝜀
𝑑𝑇
𝑑𝜀
/𝑊
/𝑇
Input  R00,  R45  and  R90  to  define  sheet  anisotropy  in  the  rolling,  45  degree  and  90 
degree direction. 
Barlat and Lian’s [1989] anisotropic yield criterion Φ for plane stress is defined as: 
𝑚 
Φ = 𝑎|𝐾1 + 𝐾2|𝑚 + 𝑎|𝐾1 − 𝐾2|𝑚 + 𝑐|2𝐾2|𝑚 = 2𝜎𝑌
for  face  centered  cubic  (FCC)  materials  exponent  m = 8  is  recommended  and  for  body 
centered cubic (BCC) materials m = 6 may be used.  Detailed description on the criterion 
can be found in *MAT_036 manual pages.
On Yoshida nonlinear kinematic hardening model: 
Background. 
The  Yoshida’s  model  accounts  for  cyclic  plasticity  including  Bauschinger  effect  and 
cyclic  hardening  behavior.    For  detailed  Yoshida’s  theory  of  nonlinear  kinematic 
hardening  rule  and  definitions  of  material  constants  CB,  Y,  SC,  K,  RSAT,  SB,  and  H, 
refer  to  Remarks  in  *MAT_125  manual  pages  and  in  the  original  paper,  “A  model  of 
large-strain  cyclic  plasticity  describing  the  Baushinger  effect  and  workhardening  stagnation”, 
by Yoshida, F.  and Uemori, T.,  Int.  J.  Plasticity, vol.  18, 661-689, 2002. 
Further  improvements  in  the  original  Yoshida’s  model,  as  described  in  a  paper 
“Determination of Nonlinear Isotropic/Kinematic Hardening Constitutive Parameter for AHSS 
using Tension and Compression Tests”, by Shi, M.F., Zhu, X.H., Xia, C., and Stoughton, T., 
in  NUMISHEET  2008  proceedings,  137-142,  2008,  included  modifications  to  allow  work 
hardening  in  large  strain  deformation  region,  avoiding  the  problem  of  earlier 
saturation, especially for Advanced High Strength Steel (AHSS).  These types of steels 
exhibit  continuous  strain  hardening  behavior  and  a  non-saturated  isotropic  hardening 
function.  As described in the paper, the evolution equation for R (a part of the current 
radius of the bounding surface in deviatoric stress space), as is with the saturation type 
of isotropic hardening rule proposed in the original Yoshida model, 
is modified as, 
𝑅̇ = 𝑚(𝑅sat − 𝑅)𝑝̇ 
𝑅 = RSAT × [(𝐶1 + 𝜀̅𝑝)𝑐2 − 𝐶1
𝑐2] 
For  saturation  type  of  isotropic  hardening  rule,  set  IOPT = 0,  applicable  to  most  of 
Aluminum sheet materials.  In addition, the paper provides detailed variables used for 
this  material  model  for  DDQ,  HSLA,  DP600,  DP780  and  DP980  materials.    Since  the 
symbols  used  in  the  paper  are  different  from  what  are  used  here,  the  following  table 
provides  a  reference  between  symbols  used  in  the  paper  and  variables  here  in  this 
keyword: 
B 
CB 
Y 
Y 
C 
SC 
m 
K 
K 
Rsat 
b 
SB 
h 
H 
e0 
C1 
N 
C2
b: R90
For shells, define vector 
a, so,
c = n
b = c × a
a = b × c
a: rolling direction R00
v × n
For shells, define vector 
v, so,
c = n
a = v × n
b = n × a
AOPT = 2
AOPT = 3
Figure M226-1.  Defining sheet metal rolling direction. 
Using the modified formulation and the material properties provided by the paper, the 
predicted  and  tested  results  compare  very  well  both  in  a  full  cycle  tension  and 
compression  test  and  in  a  pre-strained  tension  and  compression  test,  according  to  the 
paper.    A  set  of  experiments  are  required  to  fit  (optimize)  the  Yoshida  material 
constants, and these experiments include a uniaxial tension test (used for HLCID) to a 
sufficiently large strain range, a full cycle tension and compression test and a multiple 
cycle tension and compression test. 
Defining the rolling direction of a sheet metal. 
The variable AOPT is used to define the rolling direction of the sheet metals.  For shells, 
AOPT  of  2  or  3  are  relevant.    When  AOPT = 2,  define  vector  components  of  a  in  the 
direction  of  the  rolling  (R00);  when  AOPT = 3,  define  vector  components  of  v 
perpendicular to the rolling direction, as shown in Figure M226-1. 
Application. 
Application of the modified Yoshida’s hardening rule in the metal forming industry has 
shown  significant  improvement  in  springback  prediction  accuracy,  which  is  a  pre-
requisite for a successful stamping tool compensation, especially for AHSS type of sheet 
materials.
Figure M226-2.  The NUMISHEET 2005 cross member and section definition.
In  an  example  shown  in  Figure  M226-2,  springback  simulation  was  performed 
following  drawing  and  trimming  on  the  NUMISHEET  2005  cross  member  for 
aluminum alloy AL5182-O, using *MAT_226.  In Figure M226-3, springback shape was 
recovered  from  section  A-A  (Figure  M226-2),  and  compared  with  those  results  from 
simulation  using  *MAT_037  and  *MAT_125.    Though  all  are  remarkably  close,  results 
with *MAT_226 on the cross section (Y = -370 mm) show better springback correlation 
to the measured test data than those with *MAT_125 and *MAT_37. 
To  improve  convergence,  it  is  recommended  that  *CONTROL_IMPLICIT_FORMING 
type ‘1’ be used when conducting springback simulation. 
A Failure Criterion for Nonlinear Strain Paths (NLP): 
The NLP failure criterion and corresponding post processing procedures are described 
in  the  entries  for  *MAT_036  and  *MAT_037.    The  history  variables  for  every  element 
stored in d3plot files include: 
1.  Formability Index (F.I.): #1 
2.  Strain ratio (in-plane minor strain/major strain): #2 
3.  Effective strain from the planar isotropic assumption: #3 
The entire time history can be  plotted using Post/History menu in  LS-PrePost v4.0.  To 
enable  the  output  of  these  history  variables  to  the  d3plot  files,  NEIPS  on  the  *DATA-
BASE_EXTENT_BINARY card must be set to at least 3.  When plotting the formability 
index, first select the history var #1 from the Misc in the FriComp menu.  The pull-down 
menu  under  FriComp  can  be  used  to  select  minimum  value  ‘Min’  for  necking  failure 
determination  (refer  to  Tharrett  and  Stoughton’s  paper  in  2003  SAE  2003-01-1157).    In 
FriRang, the option None is to be selected in the pull-down menu next to Avg.  Lastly, set 
the  simulation  result  to  the  last  state  in  the animation  tool  bar.    The  index  value ranges 
from 0.0 to 1.5.  The non-linear forming limit is reached when the index reaches 1.0.
A  partial  keyword  example  is  listed  below  when  the  option  NLP  is  used.    In  this 
example,  the  traditional  Forming  Limit  Diagram  (FLD)  which  handles  only  the  linear 
strain paths is defined by load curve ID 213. 
*MAT_KINEMATIC_HARDENING_BARLAT89_NLP 
$#     mid        ro         e        pr         m       r00       r45       r90 
         1 2.8900E-9    7.0E+4     0.333       8.0     0.699     0.776     0.775 
$#      cb         y        sc         k      rsat        sb         h     hlcid 
     122.3     110.2     577.5      12.0     201.7      16.5      0.16         0 
$#    aopt      iopt        c1        c2      IFLD 
         2         0                           213 
$#      xp        yp        zp        a1        a2        a3 
     0.000     0.000     0.000  1.000000     0.000     0.000 
$#      v1        v2        v3        d1        d2        d3      beta 
     0.000     0.000     0.000     0.000     0.000     0.000     0.000 
*DEFINE_CURVE 
213 
-0.300,0.36 
-0.200,0.32 
-0.114,0.266 
-0.058,0.223 
0.026,0.181 
0.036,0.181 
0.111,0.211 
0.147,0.23 
0.215,0.27 
0.263,0.278 
Revision information: 
This material model is available starting in Revision 57717.  The NLP option is available 
starting in Revision 95599.
AL5182 springback comparison among 
test data/M226/M125/M37 at section A-A (Y=-370mm)
-100
-50
20
50
100
150
200
Experiments
M226 m=8
M125
M37
1.3 mm
100
120
140
160
Figure  M226-3.    Springback  prediction  with  *MAT_226  (Material  properties
courtesy of Ford Motor Company Research and Innovation Laboratory).
*MAT_230 
This  is  Material  Type  230.    This  is  a  perfectly-matched  layer  (PML)  material  —  an 
absorbing layer material used to simulate wave propagation in an unbounded isotropic 
elastic  medium  —  and  is  available  only  for  solid  8-node  bricks  (element  type  2).    This 
material  implements  the  3D  version  of  the  Basu-Chopra  PML  [Basu  and  Chopra 
(2003,2004), Basu (2009)]. 
5 
6 
7 
8 
Card 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
Default 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
MID 
RO 
E 
PR 
Remarks: 
1.  A layer of this material may be placed at a boundary of a bounded domain to 
simulate unboundedness of the domain at that boundary: the layer absorbs and 
attenuates  waves  propagating  outward  from  the  domain,  without  any  signifi-
cant  reflection  of  the  waves  back  into  the  bounded  domain.    The  layer  cannot 
support any static displacement.  
2. 
It is assumed the material in the bounded domain near the layer is, or behaves 
like,  an  isotropic  linear  elastic  material.    The  material  properties  of  the  layer 
should be set to the corresponding properties of this material.  
3.  The layer should form a cuboid box around the bounded domain, with the axes 
of the box aligned with the coordinate axes.  Various faces of this  box may be 
open,  as  required  by  the  geometry  of  the  problem,  e.g.,  for  a  half-space  prob-
lem, the “top” of the box should be open.
4. 
Internally, LS-DYNA will partition the entire PML into regions which form the 
“faces”,  “edges”  and  “corners”  of  the  above  cuboid  box,  and  generate  a  new 
material for each region.  This partitioning will be visible in the d3plot file.  The 
user may safely ignore this partitioning. 
5.  The layer should have 5-10 elements through its depth.  Typically, 5-6 elements 
are sufficient if the excitation source is reasonably distant from the layer, and 8-
10 elements if it is close.  The size of the elements should be  similar to that of 
elements in the bounded domain near the layer, and should be small enough to 
sufficiently discretize all significant wavelengths in the problem. 
6.  The nodes on the outer boundary of the layer should be fully constrained.  
7.  The stress and strain values reported by this material do not have any physical 
significance.
*MAT_PML_ELASTIC_FLUID 
This  is  Material  Type  230_FLUID.    This  is  a  perfectly-matched  layer  (PML)  material 
with a pressure fluid constitutive law, to be used in a wave-absorbing layer adjacent to 
a fluid material (*MAT_ELASTIC_FLUID) in order to simulate wave propagation in an 
unbounded fluid medium.  See the Remarks sections of *MAT_PML_ELASTIC (*MAT_-
230) and *MAT_ELASTIC_FLUID (*MAT_001_FLUID) for further details. 
5 
6 
7 
8 
Card 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
K 
F 
4 
VC 
F 
Default 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
MID 
RO 
K 
VC 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Bulk modulus 
Tensor viscosity coefficient
*MAT_PML_ACOUSTIC 
This  is  Material  Type  231.    This  is  a  perfectly-matched  layer  (PML)  material  —  an 
absorbing layer material used to simulate wave propagation in an unbounded acoustic 
medium  —  and  can  be  used  only  with  the  acoustic  pressure  element  formulation 
(element  type  14).    This  material  implements  the  3D  version  of  the  Basu-Chopra  PML 
for anti-plane motion [Basu and Chopra (2003,2004), Basu (2009)].  
4 
5 
6 
7 
8 
Card 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
C 
F 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Sound speed 
MID 
RO 
C 
Remarks: 
1.  A layer of this material may be placed at a boundary of a bounded domain to 
simulate unboundedness of the domain at that boundary: the layer absorbs and 
attenuates  waves  propagating  outward  from  the  domain,  without  any  signifi-
cant  reflection  of  the  waves  back  into  the  bounded  domain.    The  layer  cannot 
support any hydrostatic pressure. 
2. 
It is assumed the material in the bounded domain near the layer is an acoustic 
material.  The material properties of the layer should be set to the correspond-
ing properties of this material.  
3.  The layer should form a cuboid box around the bounded domain, with the axes 
of the box aligned with the coordinate axes.  Various faces of this  box may be 
open,  as  required  by  the  geometry  of  the  problem,  e.g.,  for  a  half-space  prob-
lem, the “top” of the box should be open.
4. 
Internally, LS-DYNA will partition the entire PML into regions which form the 
“faces”,  “edges”  and  “corners”  of  the  above  cuboid  box,  and  generate  a  new 
material for each region.  This partitioning will be visible in the d3plot file.  The 
user may safely ignore this partitioning. 
5.  The layer should have 5-10 elements through its depth.  Typically, 5-6 elements 
are sufficient if the excitation source is reasonably distant from the layer, and 8-
10 elements if it is close.  The size of the elements should be  similar to that of 
elements in the bounded domain near the layer, and should be small enough to 
sufficiently discretize all significant wavelengths in the problem. 
6.  The nodes on the outer boundary of the layer should be fully constrained.  
7.  The  pressure  values  reported  by  this  material  do  not  have  any  physical 
significance.
*MAT_BIOT_HYSTERETIC 
This  is  Material  Type  232.    This  is  a  Biot  linear  hysteretic  material,  to  be  used  for 
modeling the nearly-frequency-independent viscoelastic behaviour of soils subjected to 
cyclic loading, e.g.  in soil-structure interaction analysis [Spanos and Tsavachidis (2001), 
Makris  and  Zhang  (2000),  Muscolini,  Palmeri  and  Ricciardelli  (2005)].    The  hysteretic 
damping  coefficient  for  the  model  is  computed  from  a  prescribed  damping  ratio  by 
calibrating  with  an  equivalent  viscous  damping  model  for  a  single-degree-of-freedom 
system.    The  damping  increases  the  stiffness  of  the  model  and  thus  reduces  the 
computed time-step size. 
Card 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
ZT 
F 
6 
FD 
F 
7 
8 
Default 
none 
none 
none 
none 
0.0 
3.25 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
Damping ratio 
Dominant excitation frequency in Hz 
  VARIABLE   
MID 
RO 
E 
PR 
ZT 
FD 
Remarks: 
1.  The stress is computed as a function of the strain rate as 
𝜎(𝑡) = ∫ 𝐶𝑅(𝑡 − 𝜏)𝜀̇(𝜏)
𝑑𝜏 
where
𝐶𝑅(𝑡) = 𝐶 [1 +
2𝜂
𝐸1(𝛽𝑡)] 
with  𝐶 being the elastic isotropic constitutive tensor, 𝜂 the hysteretic damping 
factor,  and  𝛽 = 2𝜋𝑓𝑑/10,  where  𝑓𝑑  is  the  dominant  excitation  frequency  in  Hz.  
The function 𝐸1 is given by 
∞
𝐸1(𝑠) = ∫
e−𝜉
𝑑𝜉
For  efficient  implementation,  this  function  is  approximated  by  a  5-term  Prony 
series as 
𝐸1(𝑠) ≈ ∑ 𝑏𝑘e𝑎𝑘𝑠
𝑘=1
such that 𝑏𝑘 > 0. 
2.  The hysteretic damping factor 𝜂 is obtained from the prescribed damping ratio 
𝜍 as  
𝜂 = 𝜋𝜍/atan(10) = 2.14𝜍 
by assuming that, for a single degree-of-freedom system, the energy dissipated 
per cycle by the hysteretic material is the same as that by a viscous damper, if 
the excitation frequency matches the natural frequency of the system. 
3.  The consistent Young’s modulus for this model is given by  
where 
𝐸𝑐 = 𝐸 [1 +
2𝜂
𝑔] 
𝑔 = ∑ 𝑏𝑘
𝑘=1
𝑎𝑘𝛽Δ𝑡𝑛
[exp(𝑎𝑘𝛽Δ𝑡𝑛) − 1]
Because 𝑔 > 0, the computed element time-step size is smaller than that for the 
corresponding  elastic  element.    Furthermore,  the  time-step  size  computed  at 
any time depends on the previous time-step size.  It can be demonstrated that 
the  new  computed  time-step  size  stays  within  a  narrow  range  of  the  previous 
time-step  size,  and  for  a  uniform  mesh,  converges  to  a  constant  value.    For 
𝑓𝑑 = 3.25Hz  and  𝜍 = 0.05,  the  percentage  decrease  in  time-step  size  can  be  ex-
pected to be about 12-15% for initial time-step sizes of less than 0.02 secs, and 
about 7-10% for initial time-step sizes larger than 0.02 secs. 
4.  The  default  value  of  the  dominant  frequency  is  chosen  to  be  valid  for  earth-
quake excitation.
*MAT_CAZACU_BARLAT 
This is Material Type 233.  This material model is for Hexagonal Closed Packet (HCP) 
metals  and  is  based  on  the  work  by  Cazacu  et  al.    (2006).    This  model  is  capable  of 
describing  the  yielding  asymmetry  between  tension  and  compression  for  such 
materials.    Moreover,  a  parameter  fit  is  optional  and  can  be  used  to  find  the  material 
parameters  that  describe  the  experimental  yield  stresses.    The  experimental  data  that 
the user should supply consists of yield stresses for tension and compression in the 00 
direction, tension in the 45 and the 90 directions, and a biaxial tension test. 
Available options include: 
<BLANK> 
MAGNESIUM 
Including  MAGNESIUM  invokes  a  material  model  developed  by  the  USAMP 
consortium to simulate cast Magnesium under impact loading.  The model includes rate 
effects having a tabulated failure model including equivalent plastic strain to failure as 
a  function  of  stress  triaxiality  and  effective  plastic  strain  rate.    Element  erosion  will 
occur  when  the  number  of  integration  points  where  the  damage  variable  has  reached 
unity reaches some specified threshold (NUMINT).  Alternatively a Gurson type failure 
model can be activated, which requires less experimental data. 
The  input  of  the  hardening  curve  for  MAT_233  requires  the  user  to  provide  the 
evolution  of  the  Cazacu-Barlat  effective  stress  as  a  function  of  the  energy  conjugate 
plastic  strain.    With  the  MAGNESIUM  option  an  alternative  option  for  the  hardening 
curve  is  available:  von  Mises  effective  stress  as  a  function  of  equivalent  plastic  strain, 
which is energy conjugate to the von Mises stress. 
Finnally  the  MAGNESIUM  option  allows  for  distortional  hardening  by  providing 
hardening  curves  as  measured  in  tension  and  compression  tests.    This  option  is 
however incompatible with the activation of rate effects (visco-plasticity). 
With the MAGNESIUM option this material model is also available for solid elements. 
NOTE: Activating the MAGNESIUM options requires setting 
HR = 3 and FIT = 0.0.  (Also see below)
Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
Variable 
Type 
1 
A 
F 
  Card 3 
1 
Variable 
AOPT 
Type 
F 
2 
RO 
F 
2 
3 
E 
F 
3 
4 
PR 
F 
4 
5 
HR 
F 
5 
C11 
C22 
C33 
LCID 
F 
2 
F 
3 
I 
5 
6 
P1 
F 
6 
E0 
F 
6 
7 
P2 
F 
7 
K 
F 
7 
8 
ITER 
F 
8 
P3 
F 
8 
F 
4 
4 
A1 
F 
4 
D1 
F 
C12 
C13 
C23 
C44 
F 
F 
5 
A2 
F 
5 
D2 
F 
6 
A3 
F 
6 
D3 
F 
F 
7 
F 
8 
7 
BETA 
8 
FIT 
F 
I 
  Card 4 
1 
2 
3 
Variable 
Type 
  Card 5 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3
Magnesium Card.  Additional card for MAGNESIUM keyword option. 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LC1ID 
LC2ID 
NUMINT 
LCCID 
ICFLAG 
IDFLAG 
LC3ID 
EPSFG 
Type 
I 
I 
F 
I 
I 
I 
I 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
HR 
Material Identification number. 
Constant Mass density. 
Young’s modulus 
E.GT.0.0: constant value 
E.LT.0.0:  load  curve  ID  (–E)  which  defines  the  Young’s 
modulus as a function of plastic strain. 
Poisson’s ratio 
Hardening rules: 
HR.EQ.1.0: linear hardening (default) 
HR.EQ.2.0: exponential hardening (Swift) 
HR.EQ.3.0: load curve  
HR.EQ.4.0: exponential hardening (Voce) 
HR.EQ.5.0: exponential hardening (Gosh) 
HR.EQ.6.0: exponential hardening (Hocken-Sherby) 
HR must be set to 3 if the MAGNESIUM option is active 
P1 
Material parameter: 
HR.EQ.1.0: tangent modulus 
HR.EQ.2.0: 𝑞, coefficient for exponential hardening law (Swift)
HR.EQ.4.0: 𝑎, coefficient for exponential hardening law (Voce) 
HR.EQ.5.0: 𝑞, coefficient for exponential hardening law (Gosh)
HR.EQ.6.0: 𝑎,  coefficient 
for  exponential  hardening 
law
(Hocket-Sherby)
VARIABLE   
DESCRIPTION
P2 
Material parameter: 
HR.EQ.1.0: yield stress for the linear hardening law 
HR.EQ.2.0: 𝑛, coefficient for (Swift) exponential hardening 
HR.EQ.4.0: 𝑐, coefficient for exponential hardening law (Voce) 
HR.EQ.5.0: 𝑛, coefficient for exponential hardening law (Gosh)
HR.EQ.6.0: 𝑐,  coefficient 
for  exponential  hardening 
law
(Hocket-Sherby) 
ITER 
Iteration flag for speed: 
ITER.EQ.0.0:  fully iterative 
ITER.EQ.1.0:  fixed  at  three  iterations.    Generally,  ITER = 0.0  is 
recommended.  However, ITER = 1.0 is faster and 
may give acceptable results in most problems. 
A 
C11 
Exponent in Cazacu-Barlat’s orthotropic yield surface  (A > 1) 
Material parameter : 
FIT.EQ.1.0 or EQ.2.0: yield stress for tension in the 00 direction
FIT.EQ.0.0: 
material parameter 𝑐11 
C22 
Material parameter : 
FIT.EQ.1.0 or EQ.2.0: yield stress for tension in the 45 direction
FIT.EQ.0.0: 
material parameter 𝑐22 
C33 
Material parameter : 
FIT.EQ.1.0 or EQ.2.0: yield stress for tension in the 90 direction
FIT.EQ.0.0: material parameter 𝑐33 
LCID 
Load  curve  ID  for  the  hardening  law  (HR.EQ.3.0),  Table  ID  for
rate dependent hardening if the MAGNESIUM option is active
*MAT_CAZACU_BARLAT 
DESCRIPTION
E0 
Material parameter: 
HR.EQ.2.0: 𝜀0,  initial  yield  strain  for  exponential  hardening
law (Swift) (default = 0.0) 
HR.EQ.4.0: 𝑏, coefficient for exponential hardening (Voce) 
HR.EQ.5.0: 𝜀0,  initial  yield  strain  for  exponential  hardening
(Gosh), Default = 0.0 
HR.EQ.6.0: 𝑏,  coefficient 
for  exponential  hardening 
law
(Hocket-Sherby) 
K 
Material parameter : 
FIT.EQ.1.0 or EQ.2.0: yield  stress  for  compression  in  the  00 
direction 
FIT.EQ.0.0: 
material parameter (-1 < k<1) 
P3 
Material parameter: 
HR.EQ.5.0: 𝑝, coefficient  for exponential hardening (Gosh) 
HR.EQ.6.0: 𝑛,  exponent 
for  exponential  hardening 
law
(Hocket-Sherby
VARIABLE   
AOPT 
DESCRIPTION
Material  axes  option  . 
AOPT.EQ.0.0: locally 
orthotropic  with  material 
axes 
determined by element nodes 1, 2 and 4, as with
*DEFINE_COORDINATE_NODES, and then ro-
tated  about  the  shell  element  normal  by  the an-
gle BETA. 
AOPT.EQ.2.0: globally 
orthotropic  with  material 
axes
determined  by  vectors  defined  below,  as  with 
*DEFINED_COORDINATE_VECTOR. 
AOPT.EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating  the  material  axes  about  the  element
normal  by  an  angle  BETA,  from  a  line  in  the
plane  of  the  element  defined  by  the  cross  prod-
uct of the vector V with the element normal. 
AOPT.LT.0.0:  the absolute value of AOPT is coordinate system
ID  (CID  on  *DEFINE_COORDINATE_NODES, 
*DE-
*DEFINE_COORDINATE_SYSTEM,  or 
FINE_COORDINATE_VECTOR). 
  Available 
with the R3 release of 971 and later. 
Material  parameter.    If  parameter  identification  (FIT = 1.0)  is 
turned on C12 is not used. 
Material  parameter.    If  parameter  identification  (FIT = 1.0)  is 
turned on C13 = 0.0 
Material  parameter.    If  parameter  identification  (FIT = 1.0)  is 
turned on C23 = 0.0 
Material parameter  
FIT.EQ.1.0 or EQ.2.0: yield  stress  for  the  balanced  biaxial 
tension test. 
FIT.EQ.0.0: 
material parameter c44 
C12 
C13 
C23 
C44 
A1 - A3 
Components of vector 𝐚 for AOPT = 2.0 
V1 - V3 
Components of vector 𝐯 for AOPT = 3.0 
D1 - D3 
Components of vector 𝐝 for AOPT = 2.0
BETA 
*MAT_CAZACU_BARLAT 
DESCRIPTION
Material  angle  in  degrees  for  AOPT = 0  and  3.    NOTE,  may  be 
overridden on the element card, see *ELEMENT_SHELL_BETA 
FIT 
Flag for parameter identification algorithm: 
FIT.EQ.0.0: No  parameter  identification  routine  is  used.    The
variables K, C11, C22, C33, C44, C12, C13 and C23
are interpreted as material parameters.  FIT MUST
be set to zero if MAGNESIUM option is active 
FIT.EQ.1.0: Parameter fit is used.  The variables C11, C22, C33,
C44  and  K  are  interpreted  as  yield  stresses  in  the
00,  45,  90  degree  directions,  the  balanced  biaxial
tension and the 00 degree compression, respective-
ly. 
It is recommended to always check the d3hsp file to see 
the fitted parameters before complex jobs are submitted. 
FIT.EQ.2.0: Same  as  EQ.1.0  but  also  produce  contour  plots  of
the  yield  surface.    For  each  material  three  LS-
PrePost  ready  xy-data  files  are  created;  Con-
tour1_𝑛,  Contour2_𝑛  and  Contour3_𝑛  where  𝑛
equal the material number. 
Load  curve  ID  giving  equivalent  plastic  strain  to  failure  as  a
function  of  stress  triaxiality  or  a  table  ID  giving  plastic  strain  to
failure  as  a  function  of  Lode  parameter  and  stress  triaxiality
(solids) 
Load  curve  ID  giving  equivalent  plastic  strain  to  failure  as  a
function of equivalent plastic strain rate, the failure strain will be
computed as the product of the values on LC1ID and LC2ID 
Number  of  through  thickness  integration  points  which  must  fail 
before the element is deleted (inactive for solid elements) 
Load  curve  ID  giving effective  stress  in  function  of  plastic  strain
obtained from a compression stress, input of this load curve will
activate  distortional  hardening  and  is  NOT  compatible  with  the 
use of strain rate effects 
LC1ID 
LC2ID 
NUMINT 
LCCID
DESCRIPTION
Automated  input  conversion  flag.    If  ICFLAG = 0  then  the  load 
curves  provided  under  LCID  and  LCCID  contain  Cazacu-Barlat 
effective stress as a function of energy conjugate plastic strain.  If
ICFLAG = 1  then  both  load  curves  are  given  in  terms  of  von
Mises stress versus equivalent plastic strain 
Damage  flag.    If  IDFLAG = 0  the  failure  model  is  of  the  Johnson 
Cook type and requires LC1ID and LC2ID as additional input.  If
IDFLAG = 1 the failure model is of the Gurson type and requires 
LC3ID and EPSFG as additional input 
Load  curve giving the  critical  void  fraction of  the  Gurson  model
as  a  function  of  the  plastic  strain  to  failure  measured  in  the
uniaxial tensile test 
Plastic  strain  to  failure  measured  in  the  uniaxial  tensile  test,  this
value is used by the Gurson type failure model only. 
  VARIABLE   
ICFLAG 
IDFLAG 
LC3ID 
EPSFG 
Remarks: 
The  material  model  #233  (MAT_CAZACU_BARLAT)  is  aimed  for  modeling  materials 
with  strength  differential  and  orthotropic  behavior  under  plane  stress.    The  yield 
condition includes a parameter 𝑘 that describes the asymmetry between yield in tension 
and  compression.    Moreover,  to  include  the  anisotropic  behavior  the  stress  deviator  𝐒 
undergoes a linear transformation.  The principal values of the Cauchy stress deviator 
are  substituted  with  the  principal  values  of  the  transformed  tensor 𝐙,  which  is 
represented as a vector field, defined as: 
where 
nents𝑆𝐼 = (𝑠11, 𝑠22, 𝑠33, 𝑠12), 
the 
𝐒is 
field 
𝐙 = 𝐂𝐒
(233.1)
comprised 
of 
the 
four 
stresses 
deviator 
𝐬 = σ −
tr(σ)δ, 
where tr(σ) is the trace of the Cauchy stress tensor and δ is the Kronecker delta.  For the 
2D  plane  stress  condition,  the  orthotropic  condition  gives  7  independent  coefficients.  
The tensor 𝐂 is represented by the 4𝑥4 matrix 
𝐶𝐼𝐽 =
𝑐12
𝑐22
𝑐23
𝑐13
𝑐23
𝑐33
𝑐11
𝑐12
𝑐13
⎜⎜⎜⎜⎜⎛
⎝
⎟⎟⎟⎟⎟⎞
. 
𝑐44⎠
The principal values of 𝐙 are denoted Σ1, Σ2, Σ3 and are given as the eigenvalues to the 
matrix composed by the components Σ𝑥𝑥, Σ𝑦𝑦, Σ𝑧𝑧, Σ𝑥𝑦through
where 
Σ1 =
Σ2 =
(Σ𝑥𝑥 + Σ𝑦𝑦 + √(Σ𝑥𝑥 − Σ𝑦𝑦)
+ 4Σ𝑥𝑦
2 ) , 
(Σ𝑥𝑥 + Σ𝑦𝑦 − √(Σ𝑥𝑥 − Σ𝑦𝑦)
+ 4Σ𝑥𝑦
2 ) , 
Σ3 = Σ𝑧𝑧 
3Σ𝑥𝑥 = (2𝑐11 − 𝑐12 − 𝑐13)𝜎𝑥𝑥 + (−𝑐11 + 2𝑐12 − 𝑐13)𝜎𝑦𝑦, 
3Σ𝑦𝑦 = (2𝑐12 − 𝑐22 − 𝑐23)𝜎𝑥𝑥 + (−𝑐12 + 2𝑐22 − 𝑐23)𝜎𝑦𝑦, 
3Σ𝑧𝑧 = (2𝑐13 − 𝑐23 − 𝑐33)𝜎𝑥𝑥 + (−𝑐13 + 2𝑐23 − 𝑐33)𝜎𝑦𝑦, 
Σ𝑥𝑦 = 𝑐44𝜎12 
Note that the symmetry of Σ𝑥𝑦 follows from the symmetry of the Cauchy stress tensor. 
The yield condition is written on the following form: 
𝑓 (Σ, 𝑘, 𝜀ep) = 𝜎eff(Σ1, Σ2, Σ3, 𝑘) − 𝜎𝑦(𝜀ep) ≤ 0
(233.2)
where 𝜎𝑦(𝜀ep) is a function representing the current yield stress dependent on current 
effective plastic strain and 𝑘 is the asymmetric parameter for yield in compression and 
tension.  The effective stress 𝜎effis given by 
𝜎eff = [(|Σ1| − 𝑘Σ1)𝑎 + (|Σ2| − 𝑘Σ2)𝑎 + (∣Σ3∣ − 𝑘Σ3)𝑎]
𝐶  represent the yield stress along the rolling 
𝑇  and 𝜎00
where 𝑘 ∈ [−1,1], 𝑎 ≥ 1. Now, let 𝜎00
𝑇  and 
(00 degree) direction in tension and compression, respectively.  Furthermore let 𝜎45
𝑇 be 
𝑇  represent the yield stresses in the 45 and the 90 degree directions, and last let 𝜎𝐵
𝜎90
the  balanced  biaxial  yield  stress  in  tension.    Following  Cazacu  et  al.    (2006)  the  yield 
stresses can easily be derived. 
(233.3)
𝑎⁄  
To simplify the equations it is preferable to make the following definitions: 
Φ1 =
Φ2 =
Φ3 =
(2𝑐11 − 𝑐12 − 𝑐13)
Ψ1 =
(2𝑐12 − 𝑐22 − 𝑐23)
and 
Ψ2 =
(2𝑐13 − 𝑐23 − 𝑐33)
Ψ3 =
(−𝑐11 + 2𝑐12 − 𝑐13) 
(−𝑐12 + 2𝑐22 − 𝑐23) 
(−𝑐13 + 2𝑐23 − 𝑐33) 
The yield stresses can now be written as: 
1. 
In the 00 degree direction:
𝑇 = [
𝜎00
𝐶 = [
𝜎00
(𝜎eff)𝑎
(|Φ1| − 𝑘Φ1)𝑎 + (|Φ2| − 𝑘Φ2)𝑎 + (∣Φ3∣ − 𝑘Φ3)𝑎]
(𝜎eff)𝑎
(|Φ1| + 𝑘Φ1)𝑎 + (|Φ2| + 𝑘Φ2)𝑎 + (∣Φ3∣ + 𝑘Φ3)𝑎]
𝑎⁄
, 
𝑎⁄
2. 
In the 45 degree direction: 
𝑇 = [
𝜎45
(𝜎eff)𝑎
(|Λ1| − 𝑘Λ1)𝑎 + (|Λ2| − 𝑘Λ2)𝑎 + (∣Λ3∣ − 𝑘Λ3)𝑎]
𝑎⁄
where 
Λ1 =
Λ2 =
Λ3 =
[Φ1 + Φ2 + Ψ1 + Ψ2 + √(Φ1 + Ψ1 − Φ2 − Ψ2)2 + 4𝑐44
2 ] , 
[Φ1 + Φ2 + Ψ1 + Ψ2 − √(Φ1 + Ψ1 − Φ2 − Ψ2)2 + 4𝑐44
2 ] , 
[Φ3 + Ψ3]. 
3. 
In the 90 degree direction: 
𝑇 = [
𝜎90
(𝜎eff)𝑎
(|Ψ1| − 𝑘Ψ1)𝑎 + (|Ψ2| − 𝑘Ψ2)𝑎 + (∣Ψ3∣ − 𝑘Ψ3)𝑎]
𝑎⁄
4. 
In the balanced biaxial yield occurs when both 𝜎𝑥𝑥 and 𝜎𝑦𝑦are equal to: 
𝑇 = [
𝜎𝐵
(𝜎eff)𝑎
(|Ω1| − 𝑘Ω1)𝑎 + (|Ω2| − 𝑘Ω2)𝑎 + (∣Ω3∣ − 𝑘Ω3)𝑎]
𝑎⁄
where 
(233.4)
(233.5)
(233.6)
(233.7)
Ω1 =
Ω2 =
Ω3 =
(𝑐11 + 𝑐12 − 2𝑐13) 
(𝑐12 + 𝑐22 − 2𝑐23) 
(𝑐13 + 𝑐23 − 2𝑐33) 
Hardening laws: 
The implemented hardening laws are the following: 
1.  The Swift hardening law
2.  The Voce hardening law 
3.  The Gosh hardening law 
4.  The Hocket-Sherby hardening law 
5.  A  loading  curve,  where  the  yield  stress  is  given  as  a  function  of  the  effective 
plastic strain 
The Swift’s hardening law can be written 
where 𝑞 and 𝑛 are material parameters.  
𝜎𝑦(𝜀ep) = 𝑞(𝜀0 + 𝜀ep)
The Voce’s equation says that the yield stress can be written in the following form 
𝜎𝑦(𝜀ep) = 𝑎 − 𝑏𝑒−𝑐𝜀ep 
where  𝑎, 𝑏and  𝑐  are  material  parameters.    The  Gosh’s  equation  is  similar  to  Swift’s 
equation.  They only differ by a constant 
𝜎𝑦(𝜀ep) = 𝑞(𝜀0 + 𝜀ep)
− 𝑝 
where 𝑞, 𝜀0,  𝑛  and  𝑝  are  material  constants.    The Hocket-Sherby  equation  resemblance 
the Voce’s equation, but with an additional parameter added 
𝜎𝑦(𝜀ep) = 𝑎 − 𝑏𝑒−𝑐𝜀ep
where 𝑎, 𝑏, 𝑐 and 𝑛 are material parameters. 
Constitutive relation and material stiffness: 
The  classical  elastic  constitutive  equation  for  linear  deformations  is  the  well-known 
Hooke’s law.  This relation written in a rate formulation is given by 
𝛔̇ = 𝐃ε̇𝑒
(233.8)
where  ε𝑒  is  the  elastic  strain  and  𝐃  is  the  constitutive  matrix.    An  over  imposed  dot 
indicates  differentiation  respect  to  time.    Introducing  the  total  strain  εand  the  plastic 
strain ε𝑝, Eq.  (233.8) is classically rewritten as 
𝛔̇ = 𝐃(𝜺̇ − 𝜺̇𝑝)
(233.9)
*MAT_233 
𝐃 =
1 − 𝜈2
⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛1
⎝
1 − 𝑣
1 − 𝑣
⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞
1 − 𝑣
2 ⎠
 and (ε̇ − ε̇𝑝) =
⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛
⎝
11
𝜀̇11 − (𝜀̇𝑝)
𝜀̇22 − (𝜀̇𝑝)
22
2[𝜀̇12 − (𝜀̇𝑝)
12
2[𝜀̇13 − (𝜀̇𝑝)
13
2[𝜀̇23 − (𝜀̇𝑝)
23
⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞
]
]
]⎠
. 
The parameters 𝐸and 𝑣 are the Young’s modulus and Poisson’s ratio, respectively.  
The material stiffness 𝐃𝑝 that is needed for e.g., implicit analysis can be calculated from 
(233.9) as 
𝐃𝑝 =
∂𝛔̇
∂ε̇
.
The associative flow rule for the plastic strain is usually written 
and the consistency condition reads 
ε̇𝑝 = 𝜆̇
∂𝑓
∂𝛔
d𝑓
d𝛔
𝛔̇ +
d𝑓
dεep
ε̇ep = 0.
(233.10)
(233.10)
(233.11)
Note  that  the  centralized  “dot”  means  scalar  product  between  two  vectors.    Using 
standard  calculus  one  easily  derives  from  (1.9),  (1.10)  and  (1.11)  an  expression  for  the 
stress rate 
𝛔̇ =
𝐃 −
⎡
⎢
⎢
⎢
⎢
⎣
(𝐃
d𝑓
d𝛔
) ⋅ (𝐃
𝑑𝑓
𝑑𝛔
⋅ (𝐃
d𝑓
d𝛔
) −
)
d𝑓
⎤
⎥
d𝝈
⎥
⎥
d𝑓
⎥
dε𝑒𝑝⎦
ε̇ 
(233.12)
That means that the material stiffness used for implicit analysis is given by 
𝐃𝑝 = 𝐃 −
(𝐃
d𝑓
d𝛔
) ⋅ (𝐃
d𝑓
d𝛔
⋅ (𝐃
d𝑓
d𝝈
) −
)
d𝑓
d𝛔
d𝑓
d𝜀ep
. 
(233.13)
To  be  able  to  do  a  stress  update  we  need  to  calculate  the  tangent  stiffness  and  the 
derivative with respect to the corresponding hardening law. 
When a suitable hardening law  has been chosen the corresponding derivative is simple 
and  will  be  left  out  from  this  document.    However,  the  stress  gradient  of  the  yield 
surface is more complicated and will be outlined here.
∂𝑓
𝜕σ11
=
𝜕𝑓
𝜕Σ3
𝜕𝑓
⎜⎛1 +
⎢⎡
𝜕Σ1 ⎣
⎝
Σ𝑥𝑥 − Σ𝑦𝑦
√Σ𝑇 ⎠
⎟⎞ Φ1 +
⎜⎛1 −
⎝
Σ𝑥𝑥 − Σ𝑦𝑦
⎟⎞ Φ2
⎥⎤
⎦
√Σ𝑇 ⎠
+
𝜕𝑓
⎜⎛1 −
⎢⎡
𝜕Σ2 ⎣
⎝
Σ𝑥𝑥 − Σ𝑦𝑦
⎟⎞ Φ1 +
⎜⎛1 +
⎝
√Σ𝑇 ⎠
Σ𝑥𝑥 − Σ𝑦𝑦
√Σ𝑇 ⎠
⎟⎞ Φ2
(233.14)
⎥⎤ + Φ3 
⎦
𝜕𝑓
𝜕𝜎22
=
𝜕𝑓
⎜⎛1 +
⎢⎡
𝜕Σ1 ⎣
⎝
Σ𝑥𝑥 − Σ𝑦𝑦
⎟⎞ Ψ1 +
⎜⎛1 −
⎝
Σ𝑥𝑥 − Σ𝑦𝑦
⎟⎞ Ψ2
⎥⎤
⎦
√Σ𝑇 ⎠
√Σ𝑇 ⎠
+
𝜕𝑓
⎜⎛1 −
⎢⎡
𝜕Σ2 ⎣
⎝
Σ𝑥𝑥 − Σ𝑦𝑦
⎟⎞ Ψ1 +
⎜⎛1 +
⎝
√Σ𝑇 ⎠
Σ𝑥𝑥 − Σ𝑦𝑦
⎟⎞ Ψ2
√Σ𝑇 ⎠
and the derivative with respect to the shear stress component is 
𝜕𝑓
𝜕𝜎12
= 𝑐44
2Σ𝑥𝑦
√Σ𝑇
(
𝜕𝑓
𝜕Σ1
−
𝜕𝑓
𝜕Σ2
)
Σ𝑇 = (Σ𝑥𝑥 − Σ𝑦𝑦)
+ 4Σ𝑥𝑦
where 
and 
(233.15)
𝜕𝑓
𝜕Σ3
⎥⎤ +
⎦
Ψ3 
(233.16)
(233.17)
𝑎−1
= 𝑓 (Σ, 𝑘, 𝜀𝑒𝑝)
𝜕𝑓
𝜕Σ𝑖
(|Σ𝑖| − 𝑘Σ𝑖)𝑎−1(sgn(Σ𝑖) − 𝑘) for 𝑖 = 1,2,3 
(233.18)
Implementation: 
Assume that the stress and strain is known at time 𝑡𝑛. A trial stress σ̃𝑛+1 at time 𝑡𝑛+1 is 
calculated by assuming a pure elastic deformation, i.e., 
𝛔̃𝑛+1 = 𝛔𝑛 + 𝐃(ε𝑛+1 − ε𝑛)
(233.19)
Now,  if    𝑓 (Σ, 𝑘, 𝜀𝑒𝑝) ≤ 0  the  deformation  is  pure  elastic  and  the  new  stress  and  plastic 
strain are determined as 
𝛔𝑛+1 = 𝛔̃𝑛+1
𝑛+1 = 𝜀ep
𝜀ep
and the thickness strain increment is given by 
Δ𝜀33 = 𝜀33
𝑛+1 − 𝜀33
𝑛 = −
1 − 𝑣
(Δ𝜀11 + Δ𝜀22)
(233.20)
(233.21)
If  the  deformation  is  not  pure  elastic  the  stress  is  not  inside  the  yield  surface  and  a 
plastic iterative procedure must take place. 
1.  Set 𝑚 = 0, 𝛔(0)
𝑛+1 = 𝛔̃𝑛+1, 𝜀ep(0)
𝑛+1 = 𝜀ep
𝑛  and Δ𝜀11
𝑝(0) = Δ𝜀22
𝑝(0) = 0 
2.  Determine the plastic multiplier as 
Δ𝜆 =
d𝑓
d𝛔
𝑛+1 )
𝑛+1, 𝜀ep(𝑚)
𝑓 (𝛔(𝑚)
d𝑓
d𝛔
(σ(𝑚)
𝑛+1) ⋅ 𝐃
𝑛+1) −
(σ(𝑚)
d𝑓
d𝜀ep
𝑛+1 )
(𝜀ep(𝑚)
(233.22)
3.  Perform  a  plastic  corrector  step:  𝛔(𝑚+1)
increments in plastic strain according to 
𝑛+1 = 𝛔(𝑚)
𝑛+1 − Δ𝜆𝐃
𝑛+1
𝜀ep(𝑚+1)
= 𝜀ep(𝑚)
𝑛+1 + Δ𝜆
Δ𝜀11
𝑝(𝑛+1) = Δ𝜀11
𝑝(𝑛) + Δ𝜆
Δ𝜀22
𝑝(𝑛+1) = Δ𝜀22
𝑝(𝑛) + Δ𝜆
∂𝑓
𝜕𝜎11
𝜕𝑓
𝜕𝜎22
(𝜎(𝑚)
𝑛+1) 
(𝜎(𝑚)
𝑛+1)
4. 
If ∣𝑓 (σ(𝑚+1)
𝑛+1
, 𝜀ep
𝑛 )∣ < tol or 𝑚 = 𝑚max; stop and set  
, 
,
𝑛+1
𝑛+1
𝛔𝑛+1 = 𝛔(𝑚+1)
𝑛+1 = 𝜀ep(𝑚+1)
𝜀ep
𝑝 = Δ𝜀11
𝑝 = Δ𝜀22
Δ𝜀11
 Δ𝜀22
𝑝(𝑚+1),
𝑝(𝑚+1), 
d𝑓
d𝛔 (𝛔(𝑚)
𝑛+1)  and  find  the 
(233.23)
(233.24)
otherwise set 𝑚 = 𝑚 + 1and return to 2. 
The thickness strain increment is for plastic yield calculated as 
Δ𝜀33 = −
1 − 𝑣
(Δ𝜀11 + Δ𝜀22) − (1 −
1 − 𝑣
) (Δ𝜀11
𝑝 ) 
𝑝 + Δ𝜀22
(233.25)
The following history variables will be stored for the MAGNESIUM option: 
HV1 
HV6  
HV7 
HV8 
HV9 
equivalent plastic strain (energy conjugate to Cazacu-Barlat effective stress) 
damage 
plastic strain to failure 
number of IP that failed 
equivalent plastic strain (energy conjugate to von Mises stress)
effective stress (Cazacu-Barlat) 
HV10 
HV11  Gurson damage 
HV12 
HV13 
HV14 
void fraction 
void fraction star 
equivalent plastic strain (energy conjugate to von Mises stress)
*MAT_VISCOELASTIC_LOOSE_FABRIC 
This is Material Type 234 developed and implemented by Tabiei et al [2004].  The model 
is  a  mechanism  incorporating  the  crimping  of  the  fibers  as  well  as  the  trellising  with 
reorientation  of  the  yarns  and  the  locking  phenomenon  observed  in  loose  fabric.    The 
equilibrium  of  the  mechanism  allows  the  straightening  of  the  fibers  depending  on  the 
fiber  tension.    The  contact  force  at  the  fiber  cross  over  point  determines  the  rotational 
friction  dissipating  a  part  of  the  impact  energy.    The  stress-strain  relationship  is 
viscoelastic  based  on  a  three-element  model.    The  failure  of  the  fibers  is  strain  rate 
dependent.  *DAMPING_PART_MASS is recommended to be used in conjunction with 
this  material  model.    This  material  is  valid  for  modeling  the  elastic  and  viscoelastic 
response of loose fabric used in body armor, blade containments, and airbags. 
fill yarn
warp yarn
Figure M234-1.  Representative Volume Cell (RVC) of the model 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
Variable 
1 
TA 
Type 
F 
2 
RO 
F 
2 
W 
F 
3 
E1 
F 
3 
s 
F 
4 
E2 
F 
4 
T 
F 
5 
G12 
F 
5 
H 
F 
6 
EU 
F 
6 
S 
F 
7 
THL 
F 
7 
8 
THI 
F 
8 
EKA 
EUA 
F
4 
5 
6 
7 
8 
G23 
EKB 
AOPT 
*MAT_234 
  Card 3 
1 
Variable 
VMB 
Type 
F 
  Card 4 
1 
2 
C 
F 
2 
F 
3 
F 
4 
Variable  Not used  Not used  Not used 
A1 
Type 
  Card 5 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
F 
4 
D1 
F 
F 
5 
A2 
F 
5 
D2 
F 
6 
A3 
F 
6 
D3 
F 
7 
8 
7 
8 
  VARIABLE   
DESCRIPTION
MID 
RO 
E1 
E2 
G12 
EU 
THL 
THI 
TA 
W 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
𝐸1, Young’s modulus in the yarn axial-direction. 
𝐸2, Young’s modulus in the yarn transverse-direction. 
𝐺12, Shear modulus of the yarns. 
Ultimate strain at failure. 
Yarn locking angle. 
Initial braid angle. 
Transition angle to locking. 
Fiber width.
VARIABLE   
DESCRIPTION
S 
T 
H 
S 
EKA 
EUA 
VMB 
C 
G23 
Ekb 
AOPT 
Span between the fibers. 
Real fiber thickness. 
Effective fiber thickness. 
Fiber cross-sectional area. 
Elastic constant of element "a". 
Ultimate strain of element "a". 
Damping coefficient of element "b". 
Coefficient of friction between the fibers. 
transverse shear modulus. 
Elastic constant of element "b" 
Material  axes  option  . 
AOPT.EQ.0.0:  locally 
orthotropic  with  material 
axes
determined by element nodes 1, 2 and 4, as with
*DEFINE_COORDINATE_NODES. 
AOPT.EQ.2.0: globally 
orthotropic  with  material 
axes
determined  by  vectors  defined  below,  as  with
*DEFINED_COORDINATE_VECTOR. 
AOPT.EQ.3.0: locally  orthotropic  material  axes  defined  by  the
cross  product  of  the  vector  V  with  the  element 
normal. 
AOPT.LT.0.0:  the absolute value of AOPT is coordinate system
ID  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM,  or 
*DE-
FINE_COORDINATE_VECTOR). 
  Available 
with the R3 release of 971 and later.
45o
45o
a)
b)
min
min
c)
Figure    M234-2.    Plain  woven  fabric  as  trellis  mechanism:  a)  initial  state;  b)
slightly stretched in bias direction; c) stretched to locking. 
Remarks: 
The  parameters  of  the  Representative  Volume  Cell  (RVC)  are:  the  yarn  span,  s,  the 
fabric thickness, t, the yarn width, w, and the yarn cross-sectional area, 𝐴.  The initially 
orthogonal  yarns    are  free  to  rotate    up  to  some 
angle and after that the lateral contact between the yarns causes the locking of the trellis 
mechanism and the packing of the yarns .The minimum braid angle, 
𝜃min,  can  be  calculated  from  the  geometry  and  the  architecture  of  the  fabric  material 
having the yarn width, 𝑤, and the span between the yarns, 𝑠: 
sin(2𝜃min) =
The  other  constrain  angles  as  the  locking  range  angle,  𝜃lock,  and  the  maximum  braid 
angle, 𝜃max,  are easy to be determined then: 
𝜃𝑙𝑜𝑐𝑘 = 45° − 𝜃min  ,      𝜃max = 45° + 𝜃lock   
The  material  behavior  of  the  yarn  can  be  simply  described  by  a  combination  of  one 
Maxwell element without the dashpot and one Kelvin-Voigt element.  The 1-D model of 
viscoelasticity  is  shown  in  the  following  figure. 
  The  differential  equation  of 
viscoelasticity  of  the  yarns  can  be  derived  from  the  model  equilibrium  as  in  the 
following equation: 
(𝐾𝑎 + 𝐾𝑏)𝜎 + 𝜇𝑏𝜎̇ = 𝐾𝑎𝐾𝑏𝜀 + 𝜇𝑏𝐾𝑎𝜀̇
σ, ε
Ka
σ , ε
σ , ε
Kb
σ, ε
Figure M234-3.  Three-element visvoelasticity model 
The  input  parameters  for  the  viscoelasticity  model  of  the  material  are  only  the  static 
Young’s modulus E1, the Hookian spring coefficient (EKA) 𝐾𝑎, the viscosity coefficient 
(VMB)  𝜇𝑏,  the  static  ultimate  strain  (EU)  𝜀max,  and  the  Hookian  spring  ultimate  strain 
(EUA)𝜀𝑎max.  The other parameters can be obtained as follows: 
𝐾𝑏 =
𝜀𝑏max =
𝐾𝑎𝐸1
𝐾𝑎 − 𝐸1
𝐾𝑎 − 𝐸1
𝐾𝑎
𝜀max 
Applying the Eq.  (18) for the fill and the warp yarns, we obtain the stress increments in 
the yarns, Δ𝜎𝑓  and Δ𝜎𝑤,.  The stress in the yarns is updated for the next time step:  
(𝑛),
(𝑛) 
(𝑛+1) = 𝜎𝑤
𝜎𝑤
(𝑛) + Δ𝜎𝑤
(𝑛+1) = 𝜎𝑓
𝜎𝑓
(𝑛) + Δ𝜎𝑓
We can imagine that the RVC is smeared to the parallelepiped in order to transform the 
stress  acting  on  the  yarn  cross-section  to  the  stress  acting  on  the  element  wall.    The 
thickness of the membrane shell element used should be equal to the effective thickness, 
𝑡𝑒, that can be found by dividing the areal density of the fabric by its mass density.  The 
in-plane  stress  components  acting  on  the  RVC  walls  in  the  material  direction  of  the 
yarns are calculated as follows for the fill and warp directions: 
(𝑛+1)𝑆
2𝜎𝑓
(𝑛+1) =
𝜎𝑓11
𝑠𝑡𝑒
(𝑛) + 𝛼𝐸2Δ𝜀𝑓22
(𝑛+1) = 𝜎𝑓22
𝜎𝑓22
(𝑛)
(𝑛+1) = 𝜎𝑓12
𝜎𝑓12
(𝑛) + 𝛼𝐺12Δ𝜀𝑓12
(𝑛)
2𝜎𝑤
𝜎𝑤11
(𝑛+1) =
(𝑛+1)𝑆
𝑠𝑡𝑒
(𝑛) + 𝛼𝐸2Δ𝜀𝑤22
(𝑛+1) = 𝜎𝑤22
𝜎𝑤22
(𝑛)
(𝑛+1) = 𝜎𝑤12
𝜎𝑤12
(𝑛) + 𝛼𝐺12Δ𝜀𝑤12
(𝑛)
lock
lock
Δθ
Δθ
min
45o
max
Figure  M234-4.  The lateral contact factor as a function of average braid angle
θ. 
where E2 is the transverse Young’s modulus of the yarns, 𝐺12 is the longitudinal shear 
modulus, and α is the lateral contact factor.  The lateral contact factor is zero when the 
trellis mechanism is open and unity if the mechanism is locked with full lateral contact 
between the yarns.  There is a transition range, Δ𝜃 × TA, of the average braid angle 𝜃 in 
which the lateral contact factor, 𝛼, is a linear  function of the average braid angle.  The 
graph of the function 𝛼(𝜃) is shown in Fig. M234-4.
*MAT_MICROMECHANICS_DRY_FABRIC 
This  is  Material  Type  235  developed  and  implemented  by  Tabiei  et  al  [2001].    The 
the 
material  model  derivation  utilizes 
homogenization  technique  usually  used  in  composite  material  models.    The  model 
accounts for reorientation of the yarns and the fabric architecture.  The behavior of the 
flexible  fabric  material  is  achieved  by  discounting  the  shear  moduli  of  the  material  in 
free  state,  which  allows  the  simulation  of  the  trellis  mechanism  before  packing  the 
yarns.    This  material  is  valid  for  modeling  the  elastic  response  of  loose  fabric  used  in 
inflatable structures, parachutes, body armor, blade containments, and airbags. 
the  micro-mechanical  approach  and 
2 
RO 
F 
2 
3 
E1 
F 
3 
4 
E2 
F 
4 
5 
6 
7 
8 
G12 
G23 
V12 
V23 
F 
5 
F 
6 
F 
7 
F 
8 
THI 
THL 
BFI 
BWI 
DSCF 
CNST 
ATLR 
F 
2 
F 
3 
F 
4 
F 
5 
Variable 
VMB 
VME 
TRS 
FFLG 
AOPT 
Type 
F 
  Card 4 
1 
F 
2 
F 
3 
F 
4 
Variable  Not used  Not used  Not used 
A1 
Type 
F 
F 
5 
A2 
F 
F 
7 
F 
8 
7 
8 
F 
6 
6 
A3 
F 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
Variable 
1 
XT 
Type 
F 
  Card 3
Variable 
1 
V1 
Type 
F 
*MAT_MICROMECHANICS_DRY_FABRIC 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
7 
8 
  VARIABLE   
DESCRIPTION
MID 
RO 
E1 
E2 
G12 
G23 
V12 
V23 
XT 
THI 
THL 
BFI 
BWI 
DSCF 
CNST 
ATLR 
VME 
VMS 
TRS 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
𝐸1, Young’s modulus of the yarn in axial-direction. 
𝐸2, Young’s modulus of the yarn in transverse-direction. 
𝐺12, shear modulus of the yarns. 
𝐺23, transverse shear modulus of the yarns. 
Poisson’s ratio. 
Transverse Poisson’s ratio. 
Stress or strain to failure . 
Initial brade angle. 
Yarn locking angle. 
Initial undulation angle in fill direction. 
Initial undulation angle in warp direction. 
Discount factor 
Reorientation damping constant 
Angle tolerance for locking 
Viscous modulus for normal strain rate 
Viscous modulus for shear strain rate 
Transverse shear modulus of the fabric layer
Figure M235-1.  Yarn orientation schematic. 
  VARIABLE   
DESCRIPTION
FFLG 
Flag for stress-based or strain-based failure 
EQ.0: XT is a stress to failure 
NE.0:  XT is a strain to failure 
AOPT 
Material  axes  option  . 
AOPT.EQ.0.0: locally 
orthotropic  with  material 
axes
determined by element nodes 1, 2 and 4, as with
*DEFINE_COORDINATE_NODES. 
AOPT.EQ.2.0: globally 
orthotropic  with  material 
axes
determined  by  vectors  defined  below,  as  with
*DEFINED_COORDINATE_VECTOR. 
AOPT.EQ.3.0: locally  orthotropic  material  axes  defined  by  the
cross  product  of  the  vector  V  with  the  element
normal.  
AOPT.LT.0.0:  the absolute value of AOPT is coordinate system
ID  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM,  or 
*DE-
FINE_COORDINATE_VECTOR). 
  Available 
with the R3 release of 971 and later. 
A1 - A3 
Components of vector 𝐚 for AOPT = 2.0 
V1 - V3 
Components of vector 𝐯 for AOPT = 3.0 
D1 - D3 
Components of vector 𝐝 for AOPT = 2.0 
Remarks: 
The  Representative  Volume  Cell  (RVC)  approach  is  utilized  in  the  micro-mechanical 
model  development.    The  direction  of  the  yarn  in  each  sub-cell  is  determined  by  two 
angles – the braid angle, 𝜃 (the initial braid angle is 45 degrees), and the undulation angle 
of  the  yarn,  which  is  different  for  the  fill  and  warp-yarns,  𝛽𝑓   and  𝛽𝑤  (the  initial
undulations  are  normal  few  degrees),  respectively.    The  starting  point  for  the 
homogenization  of  the  material  properties  is  the  determination  of  the  yarn  stiffness 
matrices. 
The elasticity tensor is given by 
[𝐶′] = [𝑆′]−1 =
𝐸1
𝜈12
𝐸1
𝜈12
𝐸1
−
−
⎡    
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
     0
     0
     0
−
−
𝜈12
𝐸1
𝐸2
𝜈23
𝐸2
−
−
𝜈12
𝐸1
𝜈23
𝐸2
𝐸2
     0
     0
  0
  0
  0
𝜇𝐺12
  0
  0
  0
  0
     0
     0
  0
𝜇𝐺23
     0
     0
  0
  0
−1
  0
  0
  0
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
𝜇𝐺12⎦
  0
  0
where  𝐸1, 𝐸2, 𝜈12, 𝜈23, 𝐺12  and  𝐺23  are  Young’s  moduli,  Poisson’s  ratios,  and  the 
shear moduli of the yarn material, respectively. 𝜇  is a discount factor, which is function 
of  the  braid  angle,  𝜃,  and  has  value  between  𝜇0  and  1  as  shown  in  the  next  figure.  
Initially, in free stress state, the discount factor is a small value (DSCF = 𝜇0 A 1) and the 
material has very small resistance to shear deformation if any. 
45o
45o
Plain Woven Fabric: Free State 
Representative
 Volume Cell
Plain Woven Fabric: Stretched
min
min
Plain Woven Fabric: Compacted 
When  the  locking  occurs,  the  fabric  yarns  are  packed  and  they  behave  like  elastic 
media.  The discount factor is unity as shown in the next figure.  The micro-mechanical 
model is developed to account for the reorientation of the yarns up to the locking angle.  
The locking angle, 𝜃lock, can be obtained from the yarn width and the spacing parameter 
of  the  fabric  using  simple  geometrical  relationship.    The  transition  range,  Δ𝜃  (angle 
tolerance  for  locking),  can  be  chosen  to  be  as  small  as  possible,  but  big  enough  to 
prevent high frequency oscillations in transition to compacted state and depends on the 
range to the  locking  angle  and  the  dynamics of  the  simulated  problem.    Reorientation 
damping constant is defined to damp some of the high frequency oscillations.  A simple 
rate  effect  is  added  by  defining  the  viscous  modulus  for  normal  or  shear  strain  rate 
.
(VMB*𝜀11 or 22
.
 for normal components and VMS*𝜀12
 for the shear components). 
fill yarn
qf
qw
locking area
warp yarn
RVC
dn
45o
up
lock
lock
Locking Angles
lock
lock
Δθ
Δθ
dn
45o
up
Discount factor as a function of braid angle, θ
*MAT_236 
This is Material Type 236 developed by Carney, Lee, Goldberg, and Santhanam [2007].  
This  model  simulates  silicon  carbide  coating  on  Reinforced  Carbon-Carbon  (RCC),  a 
ceramic matrix and is based upon a quasi-orthotropic, linear-elastic, plane-stress model.  
Additional  constitutive  model  attributes  include  a  simple  (i.e.    non-damage  model 
based) option that can model the tension crack requirement: a “stress-cutoff” in tension.  
This option satisfies the tension crack requirements by limiting the stress in tension but 
not  compression,  and  having  the  tensile  “yielding”  (i.e.    the  stress-cutoff)  be  fully 
recoverable – not plasticity or damage based. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
Variable 
1 
PR 
Type 
F 
  VARIABLE   
MID 
2 
RO 
F 
2 
G 
F 
3 
E0 
F 
3 
4 
E1 
F 
4 
5 
E2 
F 
5 
6 
E3 
F 
6 
7 
E4 
F 
7 
8 
E5 
F 
8 
G_SCL 
TSL 
EPS_TAN
F 
F 
F 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density. 
E0 
E1 
E2 
E3 
E4 
E5 
E0, See Remarks below. 
E1, See Remarks below. 
E2, See Remarks below. 
E3, See Remarks below. 
E4, See Remarks below. 
E5, Young’s modulus of the yarn in transverse-direction.
*MAT_SCC_ON_RCC 
DESCRIPTION
PR 
G 
Poisson’s ratio. 
Shear modulus 
G_SCL 
Shear modulus multiplier (default = 1.0). 
TSL 
Tensile limit stress 
EPS_TAN 
Strain at which E = tangent to the polynomial curve. 
Remarks: 
This  model  for  the  silicon  carbide  coating  on  RCC  is  based  upon  a  quasi-orthotropic, 
linear-elastic, plane-stress model, given by: 
{⎧𝜎1
}⎫
𝜎2
𝜏12⎭}⎬
⎩{⎨
=
⎡
1 − 𝜈2
⎢
⎢
𝜈𝐸
⎢
⎢
1 − 𝜈2
     0
⎣
𝜈𝐸
1 − 𝜈2
1 − 𝜈2
     0
{⎧𝜀1
}⎫
𝜀2
𝛾12⎭}⎬
⎩{⎨
  0 
⎤
⎥
⎥
⎥
⎥
𝐺12⎦
  0
Additional  constitutive  model  requirements  include  a  simple  (i.e.    non-damage  model 
based) option that can model the tension crack requirement: a “stress-cutoff” in tension.  
This option satisfies the tension crack requirements by limiting the stress in tension but 
not  compression,  and  having  the  tensile  “yielding”  (i.e.    the  stress-cutoff)  be  fully 
recoverable – not plasticity or damage based. 
The tension stress-cutoff separately resets the stress to a limit value when it is exceeded 
in  each  of  the  two  principal  directions.    There  is  also  a  strain-based  memory  criterion 
that ensures unloading follows the same path as loading: the “memory criterion” is the 
tension  stress  assuming  that  no  stress  cutoffs  were  in  effect.    In  this  way,  when  the 
memory criterion exceeds the user-specified cutoff stress, the actual stress will be set to 
that  value.    When  the  element  unloads  and  the  memory  criterion  falls  back  below  the 
stress cutoff, normal behavior resumes.  Using this criterion is a simple way to ensure 
that unloading does not result in any hysteresis.  The cutoff criterion cannot be based on 
an effective stress value because effective stress does not discriminate between tension 
and  compression,  and  also  includes  shear.    This  means  that  the  in  plane,  1-  and  2- 
directions  must  be  modeled  as  independent  to  use  the  stress  cutoff.    Because  the 
Poisson’s ratio is not zero, this assumption is not true for cracks that may arbitrarily lie 
along  any  direction.    However,  careful  examination  of  damaged  RCC  shows  that 
generally, the surface cracks do tend to lie in the fabric directions, meaning that cracks 
tend  to  open  in  the  1-  or  the  2-  direction  independently.    So  the  assumption  of 
directional independence for tension cracks may be appropriate for the coating because 
of this observed orthotropy.
The  quasi-orthotropic,  linear-elastic,  plane-stress  model  with  tension  stress  cutoff  (to 
simulate  tension  cracks)  can  model  the  as-fabricated  coating  properties,  which  do  not 
show  nonlinearities,  but  not  the  non-linear  response  of  the  flight-degraded  material.   
Explicit finite element analysis (FEA) lends itself to nonlinear-elastic stress-strain relation 
instead  of  linear-elastic.    Thus,  instead  of  𝝈 = 𝐄𝜺,  the  modulus  will  be  defined  as  a 
function of some effective strain quantity, or 𝝈 = 𝐄(𝜺eff) ⋅ 𝜺, even though it is uncertain, 
from  the  available  data,  whether  or  not  the  coating  response  is  completely  nonlinear-
elastic, and does not include some damage mechanism. 
This nonlinear-elastic model cannot be implemented into a closed form solution or into 
an  implicit  solver;  however,  for  explicit  FEA  such  as  is  used  for  LS-DYNA  impact 
analysis,  the  modulus  can  be  adjusted  at  each  time  step  to  a  higher  or  lower  value  as 
desired.  In order to model the desired S-shape response curve of flight-degraded RCC 
coating,  a  function  of  strain  that  replicates  the  desired  response  must  be  found.    It  is 
assumed  that  the  nonlinearities  in  the  material  are  recoverable  (elastic)  and  that  the 
modulus is communicative between the 1- and 2- directions (going against the tension-
crack assumption that the two directions do not interact).  Sometimes stability can be a 
problem for this type of nonlinearity modeling, however, stability was not found to be a 
problem with the material constants used for the coating. 
The  von  Mises  strain  is  selected  for  the  effective  strain  definition  as  it  couples  the  3-
dimensional  loading  but  reduces  to  uniaxial  data,  so  that  the  desired  uniaxial 
compressive response can be reproduced.  So, 
𝜀eff =
√2
1 + 𝜈
2  
√(𝜀1 − 𝜀2)2 + (𝜀2 − 𝜀3)2 + (𝜀1 − 𝜀3)2 + 3𝛾12
where for a 2-D, isotropic shell element case, the z-direction strain is given by: 
The function for modulus is implemented as an arbitrary 5th order polynomial: 
𝜀3 =
−𝜈
1 − 𝜈
(𝜀1 + 𝜀2) 
𝐸(𝜀eff) = 𝐴0𝜀eff
5  
1 + ⋯ + 𝐴5𝜀eff
0 + 𝐴1𝜀eff
In  the  case  of  as-fabricated  material  the  first  coefficient  (A0)  is  simply  the  modulus  E, 
and the other coefficients (An > 0) are zero, reducing to a 0th order polynomial, or linear.  
To  match  the  degraded  stress-strain  compression  curve,  a  higher  order  polynomial  is 
needed.    Six  conditions  on  stress  were  used  (stress  and  its  derivative  at  beginning, 
middle, and end of the curve) to obtain a 5th order polynomial, and then the derivative 
of that equation was taken to obtain modulus as a function of strain, yielding a 4th order 
polynomial that represents the degraded coating modulus vs.  strain curve. 
For  values  of  strain  which  exceed  the  failure  strain  observed  in  the  laminate 
compression  tests,  the  higher  order  polynomial  will  no  longer  match  the  test  data.  
Therefore, after a specified effective-strain, representing failure, the modulus is defined
to be the tangent of the polynomial curve.  As a result, the stress/strain response has a 
continuous  derivative,  which  aids  in  avoiding  numerical  instabilities.    The  test  data 
does not clearly define the failure strain of the coating, but in the impact test it appears 
that  the  coating  has  a  higher  compressive  failure  strain  in  bending  than  the  laminate 
failure strain. 
The two dominant modes of loading which cause coating loss on the impact side of the 
RCC  (the  front-side)  are  in-plane  compression  and  transverse  shear.    The  in-plane 
compression is measured by the peak out of plane tensile strain, ε3.  As there is no direct 
loading  of  a  shell  element  in  this  direction,  ε3  is  computed  through  Poisson’s  relation 
1−𝑣 (𝜀1 + 𝜀2)  .    When  ε3  is  tensile,  it  implies  that  the  average  of  ε1  and  ε2  is 
𝜀3 = −𝑣
compressive.    This  failure  mode  will  likely  dominate  when  the  RCC  undergoes  large 
bending, putting the front-side coating in high compressive strains.  It is expected that a 
transverse  shear  failure  mode  will  dominate  when  the  debris  source  is  very  hard  or 
very  fast.    By  definition,  the  shell  element  cannot  give  a  precise  account  of  the 
transverse shear throughout the RCC’s thickness.  However, the Belytschko-Tsay shell 
element  formulation  in  LS-DYNA  has  a  first-order  approximation  of  transverse  shear 
that is based on the out-of-plane nodal displacements and rotations that should suffice 
to  give  a  qualitative  evaluation  of  the  transverse  shear.    By  this  formulation,  the 
transverse shear is constant through the entire shell thickness and thus violates surface-
traction  conditions.    The  constitutive  model implementation  records  the  peak value  of 
the tensile out-of-plane strain (ε3) and peak root-mean-sum transverse-shear: √𝜀13
2 .
2 + 𝜀23
*MAT_237 
This is Material Type 237.  This is a perfectly-matched layer (PML) material with a Biot 
linear hysteretic constitutive law, to be used in a wave-absorbing layer adjacent to a Biot 
hysteretic material (*MAT_BIOT_HYSTERETIC) in order to simulate wave propagation 
in  an  unbounded  medium  with  material  damping.    This  material  is  the  visco-elastic 
counterpart  of  the  elastic  PML  material  (*MAT_PML_ELASTIC).    See  the  Remarks 
*MAT_BIOT_HYSTERETIC 
sections  of 
(*MAT_232) for further details. 
*MAT_PML_ELASTIC 
(*MAT_230)  and 
Card 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
ZT 
F 
6 
FD 
F 
7 
8 
Default 
none 
none 
none 
none 
0.0 
3.25 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
E 
PR 
ZT 
FD 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
Damping ratio 
Dominant excitation frequency in Hz
*MAT_PERT_PIECEWISE_LINEAR_PLASTICITY 
This is Material Type 238.  It is a duplicate of Material Type 24  (*MAT_PIECEWISE_-
LINEAR_PLASTICITY)  modified  for  use  with  *PERTURBATION_MATERIAL  and 
solid  elements  in  an  explicit  analysis.    It  should  give  exactly  the  same  values  as  the 
original material, if used exactly the same.  It exists as a separate material type because 
of  the  speed  penalty  (an  approximately  10%  increase  in  the  overall  execution  time) 
associated with the use of a material perturbation. 
See Material Type 24  (*MAT_PIECEWISE_LINEAR_PLASTICITY) for a description of 
the  material  parameters.    All  of  the  documentation  for  Material  Type  24  applies.  
Recommend  practice  is  to  first  create  the  input  deck  using  Material  Type  24.  
Additionally,  the  CMP  variable  in  the  *PERTURBATION_MATERIAL  must  be  set  to 
affect  a  specific  variables  in  the  MAT_238  definition  as  defined  in  the  following  table; 
for example, CMP = 5 will perturb the yield stress. 
CMP value 
Material variable 
3 
5 
6 
7 
E 
SIGY 
ETAN 
FAIL
*MAT_COHESIVE_MIXED_MODE_ELASTOPLASTIC_RATE 
This  is  Material  Type  240.    This  model  is  a  rate-dependent,  elastic-ideally  plastic 
cohesive  zone  model.    It  includes  a  tri-linear  traction-separation  law  with  a  quadratic 
yield  and  damage  initiation  criterion  in  mixed-mode  loading,  while  the  damage 
evolution is governed by a power-law formulation.  It can be used only with cohesive 
element  fomulations;  see  the  variable  ELFORM  in  *SECTION_SOLID  and  *SECTION_
SHELL. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
RO 
ROFLG 
INTFAIL 
EMOD 
GMOD 
THICK 
Type 
A8 
  Card 2 
1 
F 
2 
F 
3 
Variable 
G1C_0 
G1C_INF  EDOT_G1
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
F 
F 
4 
T0 
F 
4 
5 
T1 
F 
5 
F 
6 
F 
7 
8 
EDOT_T 
FG1 
LCG1C 
F 
6 
F 
7 
F 
8 
Variable 
G2C_0 
G2C_INF  EDOT_G2
S0 
S1 
EDOT_S 
FG2 
LCG2C 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density 
ROFLG 
Flag  for  whether  density  is  specified  per  unit  area  or  volume.
ROFLG = 0  specified  density  per  unit  volume  (default),  and
ROFLG = 1  specifies  the  density  is  per  unit  area  for  controlling
the mass of cohesive elements with an initial volume of zero.
INTFAIL 
*MAT_COHESIVE_MIXED_MODE_ELASTOPLASTIC_RATE 
DESCRIPTION
The  number  of  integration  points  required  for  the  cohesive
element to be deleted.  If it is zero, the element will not be deleted
even if it satisfies the failure criterion.  The value of INTFAIL may
range from 1 to 4, with 1 the recommended value. 
EMOD 
The Young’s modulus of the material 
GMOD 
The shear modulus of the material 
THICK 
GT.0.0:  Cohesive thickness 
LE.0.0:  Initial thickness is calculated from nodal coordinates 
G1C_0 
GT.0.0:  Energy release rate GIC in Mode I 
LE.0.0:  Lower bound value of rate-dependent GIC 
G1C_INF 
EDOT_G1 
T0 
T1 
Upper  bound  value  of  rate-dependent  𝐺𝐼𝐶  (only  considered  if 
G1C_0 < 0) 
Equivalent  strain  rate  at  yield  initiation  to  describe  the  rate
dependency of GIC (only considered if G1C_0 < 0) 
GT.0.0:  Yield stress in Mode I 
LT.0.0:  Rate-dependency is considered, Parameter T0 
Parameter T1, only considered if T0 < 0: 
GT.0.0:  Quadratic logarithmic model 
LT.0.0:  Linear logarithmic model 
EDOT_T 
Equivalent  strain  rate  at  yield  initiation  to  describe  the  rate
dependency  of  the  yield  stress  in  Mode  I  (only  considered  if
T0 < 0) 
FG1 
Parameter  fG1  to  describe  the  tri-linear  shape  of  the  traction-
separation law in Mode I, see remarks. 
GT.0.0:  FG1 is ratio of fracture energies 𝐺𝐼,𝑃/𝐺𝐼𝐶 
LT.0.0:  |FG1| is ratio of displacements (𝛿𝑛2 − 𝛿𝑛1)/(𝛿𝑛𝑓 − 𝛿𝑛1)
LCG1C 
Load curve ID which defines fracture energy GIC as a function of
cohesive element thickness.  G1C_0 and G1C_INF are ignored in 
that case.
Stress
T, S
En, Et
Unloading Path
Gp
Gc
n1, δ
t1
n2, δ
t2
nf, δ
tf
n, Δ
Figure M240-1.  Trilinear traction separation law 
DESCRIPTION
GT.0.0:  Energy release rate GIIC in Mode II 
LE.0.0:  Lower bound value of rate-dependent GIIC 
  VARIABLE   
G2C_0 
G2C_INF 
Upper bound value of 𝐺𝐼𝐼𝐶 (only considered if G2C_0 < 0) 
EDOT_G2 
Equivalent  strain  rate  at  yield  initiation  to  describe  the  rate
dependency of GIIC (only considered if G2C_0 < 0) 
S0 
S1 
GT.0.0:  Yield stress in Mode II 
LT.0.0:  Rate-dependency is considered, Parameter S0 
Parameter S1, only considered if S0 < 0: 
GT.0.0:  Quadratic logarithmic model is applied 
LT.0.0:  Linear logarithmic model is applied 
EDOT_S 
Equivalent  strain  rate  at  yield  initiation  to  describe  the  rate 
dependency  of  the  yield  stress  in  Mode  II  (only  considered  if
S0 < 0) 
FG2 
Parameter  fG2  to  describe  the  tri-linear  shape  of  the  traction-
separation law in Mode II, see remarks. 
GT.0.0:  FG2 is ratio of fracture energies 𝐺𝐼𝐼,𝑃/𝐺𝐼𝐼𝐶 
LT.0.0:  |FG2| is ratio of displacements (𝛿𝑡2 − 𝛿𝑡1)/(𝛿𝑡𝑓 − 𝛿𝑡1)
Load curve ID which defines fracture energy GIIC as a function of 
cohesive element thickness.  G2C_0 and G2C_INF are ignored in 
that case. 
*MAT_240 
  VARIABLE   
LCG2C 
Remarks: 
The  model  is  a  tri-linear  elastic-ideally  plastic  Cohesive  Zone  Model,  which  was 
developed by Marzi et al.  [2009].  It looks similar to *MAT_185, but considers effects of 
plasticity and rate-dependency.  Since the entire separation at failure is plastic, no brittle 
fracture behavior can be modeled with this material type. 
The separations Δ𝑛 in normal (peel) and Δ𝑡 in tangential (shear) direction are calculated 
from the element’s separations in the integration points, 
and 
Δ𝑛 = max (un, 0) 
Δ𝑡 = √𝑢𝑡1
2 , 
2 + 𝑢𝑡2
𝑢𝑛,  𝑢𝑡1 and 𝑢𝑡2 are the separations in normal and in the both  tangential directions of the 
element coordinate system.  The total (mixed-mode) separation Δ𝑚 is determined by 
Δ𝑚 = √Δ𝑛
2 + Δ𝑡
2. 
The  initial  stiffnesses  in  both  modes  are  calculated  from  the  elastic  Young’s  and  shear 
moduli and are respectively, 
𝐸𝑛 =
𝐸𝑡 =
EMOD
THICK
GMOD
THICK
, 
where  THICK,  the  element’s  thickness,  is  an  input  parameter.    Unless  the  input 
THICK > 0  it  is  calculated  from  the  distance  between  the  initial  positions  of  the 
element’s corner nodes (Nodes 1-5, 2-6, 3-7 and 4-8, respectively). 
While  the  total  energy  under  the  traction-separation  law  is  given  by  𝐺𝐶,  one  further 
parameter is needed to describe the exact shape of the tri-linear material model.  If the 
area  (energy)  under  the  constant  stress  (plateau)  region  is  denoted  𝐺𝑃  ,  a 
parameter 𝑓𝐺 defines the shape of the traction-separation law,
for mode I loading:
0 ≤ 𝑓𝐺1 =
𝐺𝐼,𝑃
𝐺𝐼𝐶
< 1 −
𝑇2
2𝐺𝐼𝐶𝐸𝑛
< 1
for mode II  loading:
0 ≤ 𝑓𝐺2 =
𝐺𝐼𝐼,𝑃
𝐺𝐼𝐼𝐶
< 1 −
𝑆2
2𝐺𝐼𝐼𝐶𝐸𝑡
< 1
As a recommended alternative, the shape of the tri-linear model can be described by the 
following displacement ratios (triggered by negative input values for 𝑓𝐺):  
for mode I loading:
𝛿𝑛2 − 𝛿𝑛1
𝛿𝑛𝑓 − 𝛿𝑛1
0 < ∣𝑓𝐺1∣ = ∣
∣ < 1
for mode II  loading:
𝛿𝑡2 − 𝛿𝑡1
𝛿𝑡𝑓 − 𝛿𝑡1
0 < ∣𝑓𝐺2∣ = ∣
∣ < 1
While  𝑓𝐺1  and  𝑓𝐺2  are  always  constant  values,  𝑇, 𝑆, 𝐺𝐼𝐶  and  𝐺𝐼𝐼𝐶  may  be  chosen  as 
functions of an equivalent strain rate 𝜀̇𝑒𝑞, which is evaluated by 
𝜀̇𝑒𝑞 =
√𝑢̇𝑛
2 + 𝑢̇𝑡2
2 + 𝑢̇𝑡1
THICK
, 
where 𝑢̇𝑛, 𝑢̇𝑡1 and 𝑢̇𝑡2 are the velocities corresponding to the separations 𝑢𝑛, 𝑢𝑡1 and 𝑢𝑡2. 
For the yield stresses, two rate dependent formulations are implemented: 
1.  A quadratic logarithmic function: 
for mode I if T0 < 0 and T1 > 0:
𝑇(𝜀̇eq) = |T0| + |T1| [max (0, ln
𝜀̇eq
EDOT_ T
)]
for mode II  if S0 < 0 and S1 > 0:
𝑆(𝜀̇eq) = |S0| + |S1| [max (0, ln
𝜀̇eq
EDOT_ S
)]
2.  A linear logarithmic function:
for mode I if T0 < 0 and T1 < 0:
𝑇(𝜀̇eq) = |T0| + |T1|max (0, ln
𝜀̇eq
EDOT_ T
)
for mode II  if S0 < 0 and S1 < 0:
𝜀̇eq
EDOT_ S
𝑆(𝜀̇eq) = |S0| + |S1|max (0, ln
)
Alternatively, T and S can be set to constant values: 
for mode I if T0 > 0:
𝑇(𝜀̇eq) = T0
for mode II  if S0 > 0:
𝑆(𝜀̇eq) = SO
The rate-dependency of the fracture energies are given by 
if G1C_ 0 < 0:
𝐺𝐼𝐶(𝜀̇eq) = |G1C_ 0| + (G1C_ INF − |G1C_ 0|)exp (−
EDOT_ G1
𝜀̇eq
)
if G2C_ 0 < 0:
𝐺𝐼𝐼𝐶(𝜀̇eq) = |G2C_ 0| + (G2C_ INF − |G2C_ 0|)exp (−
EDOT_ G2
𝜀̇eq
)
If positive values are chosen for G1C_0 or G2C_0, no rate-dependency is considered for 
this parameter and its value remains constant as specified by the user. 
As  an  alternative,  fracture  energies  GIC  and  GIIC  can  be  defined  as  functions  of 
cohesive  element  thickness  by  using  load  curves  LCG1C  and  LCG2C.    In  that  case, 
parameters  G1C_0,  G1C_INF,  G2C_0,  and  G2C_INF  will  be  ignored  and  no  rate 
dependence is considered. 
It should be noticed, that the equivalent strain rate 𝜀̇eq is updated until Δ𝑚 > 𝛿𝑚1, then 
the model behavior depends on the equivalent strain rate at yield initiation. 
Having defined the parameters describing the single modes, the mixed-mode behavior 
is formulated by quadratic initiation criteria for both yield stress and damage initiation, 
while the damage evolution follows a Power-Law.
Traction
n1
n2
nf
Δn
t1
m1
tf
t2
Δt
m2
mf
Δm
Figure M240-2.  Trilinear mixed mode traction-separation law 
Due to reasons of readability, the following simplifications are made, 
𝑇 = 𝑇(𝜀̇eq), 𝑆 = 𝑆(𝜀̇eq), 𝐺𝐼𝐶 = 𝐺𝐼𝐶(𝜀̇eq) and 𝐺𝐼𝐼𝐶 = 𝐺𝐼𝐼𝐶(𝜀̇eq). 
The mixed-mode yield initiation displacement 𝛿𝑚1 is defined as 
𝛿𝑚1 = 𝛿𝑛1𝛿𝑡1√
1 + 𝛽2
2 + (𝛽𝛿𝑛1)2
𝛿𝑡1
, 
  are  the  single-mode  yield  initiation  displacements  and 
  is  the  mixed-mode  ratio.    Analog  to  the  yield  initiation,  the  damage  initiation 
  and  𝛿𝑡1 = 𝑆
𝐸𝑡
where  𝛿𝑛1 = 𝑇
𝐸𝑛
𝛽 =
displacement 𝛿𝑚2 is defined: 
Δ𝑡
Δ𝑛
𝛿𝑚2 = 𝛿𝑛2𝛿𝑡2√
1 + 𝛽2
2 + (𝛽𝛿𝑛2)2
, 
𝛿𝑡2
where 
𝛿𝑛2 = 𝛿𝑛1 +
𝛿𝑡2 = 𝛿𝑡1 +
𝑓𝐺1𝐺𝐼𝐶
𝑓𝐺2𝐺𝐼𝐼𝐶
. 
With 𝛾 = arccos(
⟨𝑢𝑛⟩
Δ𝑚
), the ultimate (failure) displacement 𝛿𝑚𝑓  can be written, 
𝛿𝑚𝑓 =
𝛿𝑚1(𝛿𝑚1 − 𝛿𝑚2)𝐸𝑛𝐺𝐼𝐼𝐶cos2𝛾 + 𝐺𝐼𝐶(2𝐺𝐼𝐼𝐶 + 𝛿𝑚1(𝛿𝑚1 − 𝛿𝑚2)𝐸𝑡sin2𝛾)
𝛿𝑚1(𝐸𝑛𝐺𝐼𝐼𝐶cos2𝛾 + 𝐸𝑡𝐺𝐼𝐶sin2𝛾)
. 
This  formulation  describes  a  power-law  damage  evolution  with  an  exponent  𝜂 = 1.0 
.
After  the  shape  of  the  mixed-mode  traction-separation  law  has  been  determined  by 
𝛿𝑚1, 𝛿𝑚2 and 𝛿𝑚𝑓 , the plastic separation in each element direction, 𝑢𝑛,𝑃, 𝑢𝑡1,𝑃 and 𝑢𝑡2,𝑃 can 
be calculated.  The plastic separation in peel direction is given by 
𝑢𝑛,𝑃 = max(𝑢𝑛,𝑃,Δ𝑡−1, 𝑢𝑛 − 𝛿𝑚1cos (𝛾), 0). 
In shear direction, a shear yield separation 𝛿𝑡,𝑦,  
𝛿𝑡,𝑦 = √(𝑢𝑡1 − 𝑢𝑡1,𝑃,Δ𝑡−1)2 + (𝑢𝑡2 − 𝑢𝑡2,𝑃,Δ𝑡−1)2, 
is  defined.    If  𝛿𝑡,𝑦 > 𝛿𝑚1sin𝛾,  the  plastic  shear  separations  in  the  element  coordinate 
system are updated, 
𝑢𝑡1,𝑃 = 𝑢𝑡1,𝑃,Δ𝑡−1 + 𝑢𝑡1 − 𝑢𝑡1,Δ𝑡−1 
𝑢𝑡2,𝑃 = 𝑢𝑡2,𝑃,Δ𝑡−1 + 𝑢𝑡2 − 𝑢𝑡2,Δ𝑡−1. 
In  the  formulas  above,  Δ𝑡 − 1  indicates  the  individual  value  from  the  last  time 
increment.  In case Δ𝑚 > 𝛿𝑚2, the damage initiation criterion is satisfied and a damage 
variable D increases monotonically, 
𝐷 = max (
Δ𝑚 − 𝛿𝑚2
𝛿𝑚𝑓 − 𝛿𝑚2
, 𝐷Δ𝑡−1, 0). 
When  Δ𝑚 > 𝛿𝑚𝑓 ,  complete  damage  (𝐷 = 1)  is  reached  and  the  element  fails  in  the 
corresponding integration point. 
Finally, the peel and the shear stresses in element directions are calculated, 
𝜎𝑡1 = 𝐸𝑡(1 − 𝐷)(𝑢𝑡1 − 𝑢𝑡1,𝑃) 
𝜎𝑡2 = 𝐸𝑡(1 − 𝐷)(𝑢𝑡2 − 𝑢𝑡2𝑃). 
In peel direction, no damage under pressure loads is considered if 𝑢𝑛 − 𝑢𝑛,𝑃 > 0 
otherwise, 
Reference: 
𝜎𝑛 = 𝐸𝑛(𝑢𝑛 − 𝑢𝑛,𝑃) 
𝜎𝑛 = 𝐸𝑛(1 − 𝐷)(𝑢𝑛 − 𝑢𝑛,𝑃) 
S.    Marzi,  O.    Hesebeck,  M.    Brede  and  F.    Kleiner  (2009),  A  Rate-Dependent,  Elasto-
Plastic  Cohesive  Zone  Mixed-Mode  Model  for  Crash  Analysis  of  Adhesively  Bonded 
Joints, In Proceeding: 7th European LS-DYNA Conference, Salzburg
*MAT_JOHNSON_HOLMQUIST_JH1 
This is Material Type 241.  This Johnson-Holmquist Plasticity Damage Model is useful 
for modeling ceramics, glass and other brittle materials.  This version corresponds to the 
original  version  of  the  model,  JH1,  and  Material  Type  110  corresponds  to  JH2,  the 
updated model. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
Variable 
EPSI 
Type 
F 
  Card 3 
1 
2 
RO 
F 
2 
T 
F 
2 
Variable 
EPFMIN 
EPFMAX 
Type 
F 
F 
  VARIABLE   
MID 
8 
C 
F 
8 
8 
3 
G 
F 
3 
4 
P1 
F 
4 
5 
S1 
F 
5 
6 
P2 
F 
6 
7 
S2 
F 
7 
ALPHA 
SFMAX 
BETA 
DP1 
F 
7 
F 
F 
F 
F 
3 
K1 
F 
4 
K2 
F 
5 
K3 
F 
6 
FS 
F 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Density. 
G 
P1 
S1 
P2 
S2 
Shear modulus. 
Pressure point 1 for intact material. 
Effective stress at P1. 
Pressure point 2 for intact material. 
Effective stress at P2.
Intact material
strength (D < 0)
(P1, S1)
(P2, S2)
(P3, S3)
.
ε*>1
.
ε*=1
.
ε*>1
.
ε*=1
Fractured material
strength (D ≥ 0)
ALPHA
(T, 0)
Pressure
Figure M241-1.  Strength:  equivalent stress versus pressure. 
  VARIABLE   
DESCRIPTION
C 
EPSI 
T 
Strain rate sensitivity factor. 
Quasi-static threshold strain rate.  See *MAT_015. 
Maximum  tensile  pressure  strength.    This  value  is  positive  in
tension. 
ALPHA 
Initial  slope  of  the  fractured  material  strength  curve.    See
Figure M241-1. 
SFMAX 
Maximum strength of the fractured material. 
BETA 
DP1 
Fraction  of  elastic  energy  loss  converted  to  hydrostatic  energy
(affects  bulking  pressure  (history  variable  1)  that  accompanies
damage). 
Maximum  compressive  pressure  strength.    This  value  is  positive
in compression. 
EPFMIN 
Plastic strain for fracture at tensile pressure 𝑇.  See Figure M241-2.
EPFMAX 
Plastic  strain  for  fracture  at  compressive  pressure  DP1.    See
Figure M241-1. 
K1 
K2 
First pressure coefficient (equivalent to the bulk modulus). 
Second pressure coefficient.
)
fp
(
(DP1, EPFMAX)
(T, EPFMIN)
Pressure
Figure M241-2.  Fracture strain versus pressure. 
  VARIABLE   
DESCRIPTION
K3 
FS 
Third pressure coefficient. 
Element deletion criteria. 
LT.0:  delete if  P < FS  (tensile failure). 
EQ.0: no element deletion (default). 
GT.0: delete element if  the 𝜀̅𝑝> FS. 
Remarks: 
The equivalent stress for both intact and fractured ceramic-type materials is given by 
𝜎𝑦 = (1 + 𝑐 ln 𝜀̇∗)𝜎(𝑃) 
where 𝜎(𝑃) is evaluated according to Figure M241-1. 
𝑝 (𝑃) 
𝐷 = ∑ Δ𝜀𝑝/𝜀𝑓
represents  the  accumulated  damage  (history  variable  2)  based  upon  the  increase  in 
plastic  strain  per  computational  cycle  and  the  plastic  strain  to  fracture  is  evaluated 
according to Figure M241-2. 
In undamaged material, the hydrostatic pressure is given by 
in compression and by 
𝑃 = 𝑘1𝜇 + 𝑘2𝜇2 + 𝑘3𝜇3 + 𝛥𝑃 
𝑃 = 𝑘1𝜇 + 𝛥𝑃 
in tension where 𝜇 = 𝜌 𝜌0 − 1
.  A fraction, between 0 and 1, of the elastic energy loss, 𝛽, 
is converted into hydrostatic potentiall energy (pressure).  The pressure increment, 𝛥𝑃, 
associated  with  the  increment  in  the  hydrostatic  potential  energy  is  calculated  at 
⁄
𝑓   are  the  intact  and  failed  yield  stresses  respectively.    This 
fracture,  where  𝜎𝑦  and  𝜎𝑦
pressure  increment  is  applied  both  in  compression  and  tension,  which  is  not  true  for 
JH2 where the increment is added only in compression. 
𝛥𝑃 = −𝑘1𝜇𝑓 + √(𝑘1𝜇𝑓 )
+ 2𝛽𝑘1𝛥𝑈 
𝛥𝑈 =
𝜎𝑦 − 𝜎𝑦
6𝐺
*MAT_KINEMATIC_HARDENING_BARLAT2000 
This  is  Material  Type  242.    This  model  combines  Yoshida  non-linear  kinematic 
hardening  rule  (*MAT_125)  with  the  8-parameter  material  model  of  Barlat  and  Lian 
(2003)  (*MAT_133)  to  model  metal  sheets  under  cyclic  plasticity  loading  and  with 
anisotropy in plane stress condition.  Also see manual pages in *MAT_226. 
  Card 1 
1 
Variable 
MID 
Type 
I 
2 
RO 
F 
3 
E 
F 
4 
PR 
F 
5 
6 
8 
7 
M 
F 
Default 
none 
0.0 
0.0 
0.0 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ALPHA1 
ALPHA2 
ALPHA3 
ALPHA4 
ALPHA5 
ALPHA6 
ALPHA7 
ALPHA8 
Type 
F 
F 
F 
F 
F 
F 
F 
I 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
none 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
  Card 5 
Variable 
1 
CB 
Type 
F 
2 
Y 
F 
3 
C 
F 
4 
K 
F 
5 
RSAT 
F 
6 
SB 
F 
7 
H 
F 
8 
Default 
none 
none 
none 
none 
none 
none 
none 
  Card 6 
1 
2 
3 
Variable 
AOPT 
Type 
I 
IOPT 
I 
4 
C1 
F 
5 
C2 
F 
Default 
none 
none 
0.0 
0.0 
6 
7 
8 
  Card 7 
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
3 
ZP 
F 
4 
A1 
F 
5 
A2 
F 
6 
A3 
F 
7 
8 
Default 
none 
none 
none 
none 
none 
none
Card 8 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
7 
8 
Default 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
M 
ALPHA1 
ALPHA2 
ALPHA3 
ALPHA4 
ALPHA5 
ALPHA6 
ALPHA7 
ALPHA8 
CB 
Y 
SC 
K 
RSAT 
SB 
Material identification.  A unique number must be specified. 
Mass density. 
Young’s modulus, E. 
Poisson’s ratio, ν. 
Flow potential exponent.  For face centered cubic (FCC) materials
m = 8  is  recommended  and  for  body  centered  cubic  (BCC)
materials m = 6 may be used. 
α1, material constant in Barlat’s yield equation. 
α2, material constant in Barlat’s yield equation. 
α3, material constant in Barlat’s yield equation. 
α4, material constant in Barlat’s yield equation. 
α5, material constant in Barlat’s yield equation. 
α6, material constant in Barlat’s yield equation. 
α7, material constant in Barlat’s yield equation. 
α8, material constant in Barlat’s yield equation. 
The uppercase B defined in the Yoshida’s equations. 
Anisotropic  parameter 
stagnation, defined in the Yoshida’s equations. 
associated  with  work-hardening 
The lowercase c defined in the Yoshida’s equations. 
Hardening parameter as defined in the Yoshida’s equations. 
Hardening parameter as defined in the Yoshida’s equations. 
The lowercase b as defined in the Yoshida’s equations.
H 
AOPT 
*MAT_KINEMATIC_HARDENING_BARLAT2000 
DESCRIPTION
Anisotropic  parameter 
stagnation, defined in the following Yoshida’s equations. 
associated  with  work-hardening 
Material  axes  option  : 
EQ.0.0:  locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES.  
EQ.2.0:  globally orthotropic with material axes determined by 
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR.  
EQ.3.0:  locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the 
element normal.  
LT.0.0:  the  absolute  value  of AOPT  is  a  coordinate system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available with the R3 release 
of Version 971 and later. 
IOPT 
Kinematic hardening rule flag:  
EQ.0: Original Yoshida formulation. 
EQ.1: Modified formulation.  Define C1, C2 below. 
C1, C2 
Constants used to modify R: 
𝑅 = RSAT × [(𝐶1 + 𝜀̅𝑝)𝑐2 − 𝐶1
𝑐2] 
Coordinates of point p for AOPT = 1. 
Components of vector a for AOPT = 2. 
Components of vector v for AOPT = 3. 
Components of vector d for AOPT = 2. 
XP, YP, ZP 
A1, A2, A3 
V1, V2, V3 
D1, D2, D3 
Remarks: 
1.  A  total  of  eight  parameters  (α1  to  α8)  are  needed  to  describe  the  yield  surface.  
The parameters can be determined with tensile tests in three directions and an
equal  biaxial  tension  test.    For  detailed  theoretical  background  and  material 
parameters of some typical FCC materials, please see remarks in *MAT_133 and 
Barlat’s 2003 paper. 
2.  NUMISHEET 2005 provided a complete set of the parameters of AL5182-O for 
Benchmark #2, the cross member, as below (flow potential exponent M = 8): 
α1 
0.94 
α2 
1.08 
α3 
0.97 
α4 
1.0 
α5 
1.0 
α6 
1.02 
α7 
1.03 
α8 
1.11 
3.  For  a  more  detailed  description  on  the  Yoshida  model  and  parameters,  please 
see Remarks in *MAT_226 and *MAT_125. 
4.  For information on variable AOPT please see remarks in *MAT_226.  
5.  To  improve  convergence,  it  is  recommended  that  *CONTROL_IMPLICIT_-
FORMING type ‘1’ be used when conducting springback simulation. 
6.  This  material  model  is  available  in  LS-DYNA  R5  Revision  58432  or  later 
releases.
*MAT_HILL_90 
This is Material Type 243.  This model was developed by Hill [1990] for modeling sheets 
with anisotropic materials under plane stress conditions.  This material allows the use 
of  the  Lankford  parameters  for  the  definition  of  the  anisotropy.    All  features  of  this 
model are the same as in *MAT_036, only the yield condition and associated flow rules 
are replaced by the Hill90 equations. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
Variable 
Type 
1 
M 
F 
2 
RO 
F 
2 
3 
E 
F 
3 
4 
PR 
F 
4 
5 
HR 
F 
5 
R00 / AH  R45 / BH  R90 / CH 
LCID 
F 
F 
F 
I 
6 
P1 
F 
6 
E0 
F 
7 
P2 
F 
7 
SPI 
F 
8 
ITER 
F 
8 
P3 
F 
Hardening Card.  Additional Card for M < 0. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CRC1 
CRA1 
CRC2 
CRA2 
CRC3 
CRA3 
CRC4 
CRA4 
Type 
F 
  Card 4 
1 
Variable 
AOPT 
Type 
F 
F 
2 
C 
F 
F 
5 
F 
3 
P 
F 
F 
4 
VLCID 
I 
F 
6 
FLAG 
F 
F 
7 
F
1 
2 
3 
Variable 
Type 
  Card 6 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
This card is optional. 
4 
A1 
F 
4 
D1 
F 
5 
A2 
F 
5 
D2 
F 
6 
A3 
F 
6 
D3 
F 
*MAT_243 
7 
8 
7 
8 
BETA 
F 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
USRFAIL 
Type 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus, E 
GT.0.0:  Constant value, 
LT.0.0:  Load  curve  ID = (-E)  which  defines  Young’s  Modulus 
as a function of plastic strain.  See Remark 1. 
PR 
Poisson’s ratio, ν
*MAT_HILL_90 
DESCRIPTION
HR 
Hardening rule: 
EQ.1.0:  linear (default), 
EQ.2.0:  exponential (Swift) 
EQ.3.0:  load curve or table with strain rate effects 
EQ.4.0:  exponential (Voce) 
EQ.5.0:  exponential (Gosh) 
EQ.6.0:  exponential (Hocket-Sherby) 
EQ.7.0:  load curves in three directions 
EQ.8.0:  table with temperature dependence 
EQ.9.0:  3d table with temperature and strain rate dependence 
P1 
Material parameter: 
HR.EQ.1.0:  Tangent modulus, 
HR.EQ.2.0:  k,  strength  coefficient 
hardening  
for  Swift  exponential
HR.EQ.4.0:  a, coefficient for Voce exponential hardening 
HR.EQ.5.0:  k,  strength  coefficient 
hardening 
for  Gosh  exponential
HR.EQ.6.0:  a,  coefficient 
for  Hocket-Sherby  exponential 
hardening 
HR.EQ.7.0:  load curve ID for hardening in 45 degree direction. 
See Remark 2. 
P2 
Material parameter: 
HR.EQ.1.0:  Yield stress 
HR.EQ.2.0:  n, exponent for Swift exponential hardening 
HR.EQ.4.0:  c, coefficient for Voce exponential hardening 
HR.EQ.5.0:  n, exponent for Gosh exponential hardening 
HR.EQ.6.0:  c,  coefficient 
for  Hocket-Sherby  exponential 
hardening 
HR.EQ.7.0:  load curve ID for hardening in 90 degree direction.
See Remark 2.
DESCRIPTION
ITER 
Iteration flag for speed: 
ITER.EQ.0.0:  fully iterative 
ITER.EQ.1.0:  fixed at three iterations 
*MAT_243 
M 
CRCn 
CRAn 
R00 
Generally,  ITER = 0  is  recommended.    However,  ITER = 1  is 
somewhat  faster  and  may  give  acceptable  results  in  most
problems. 
m,  exponent  in  Hill’s  yield  surface,  absolute  value  is  used  if
negative.    Typically,  m  ranges  between  1  and  2  for  low-r 
materials, such as aluminum (AA6111: m≈1.5), and is greater than 
2 for high r-values, as in steel (DP600: m≈4). 
Chaboche-Rousselier hardening parameters, see remarks. 
Chaboche-Rousselier hardening parameters, see remarks. 
R00, Lankford parameter in 0 degree direction 
GT.0.0:  Constant value, 
LT.0.0:  Load curve or Table ID = (-R00) which defines R value 
as a function of plastic strain (Curve) or as a function of
temperature and plastic strain (Table).  See Remark 3. 
R45 
R45, Lankford parameter in 45 degree direction 
GT.0.0:  Constant value, 
LT.0.0:  Load curve or Table ID = (-R45) which defines R value 
as a function of plastic strain (Curve) or as a function of
temperature and plastic strain (Table).  See  Remarks 2
and 3. 
R90 
R90, Lankford parameter in 90 degree direction 
GT.0.0:  Constant value, 
LT.0.0:  Load curve or Table ID = (-R90) which defines R value 
as a function of plastic strain (Curve) or as a function of
temperature and plastic strain (Table).  See  Remarks 2
and 3. 
AH 
BH 
a, Hill90 parameter, which is read instead of R00 if FLAG = 1. 
b, Hill90 parameter, which is read instead of R45 if FLAG = 1.
CH 
LCID 
*MAT_HILL_90 
DESCRIPTION
c, Hill90 parameter, which is read instead of R90 if FLAG = 1. 
Load curve/table ID for hardening in the 0 degree direction.  See
Remark 1. 
E0 
Material parameter 
HR.EQ.2.0:  𝜀0  for  determining  initial  yield  stress  for  Swift
exponential hardening.  (Default = 0.0) 
HR.EQ.4.0:  b, coefficient for Voce exponential hardening 
HR.EQ.5.0:  𝜀0  for  determining  initial  yield  stress  for  Gosh
exponential hardening.  (Default = 0.0) 
HR.EQ.6.0:  b,  coefficient 
for  Hocket-Sherby  exponential 
hardening 
SPI 
if 𝜀0 is zero above and HR = 2.0. (Default = 0.0) 
⁄
(𝑛−1)
EQ.0.0:  𝜀0 =
⎜⎜⎜⎛𝐸
𝑘⁄
⎝
⎟⎟⎟⎞
⎠
LE.0.02:  𝜀0 = SPI 
GT.0.02:  𝜀0 =
1 𝑛⁄
⎜⎜⎜⎛SPI
⁄
⎝
⎟⎟⎟⎞
⎠
If HR = 5.0 the strain at plastic yield is determined by an iterative
procedure based on the same principles as for HR.EQ.2.0. 
P3 
Material parameter: 
HR.EQ.5.0:  p, parameter for Gosh exponential hardening 
HR.EQ.6.0:  n,  exponent 
for  Hocket-Sherby  exponential 
hardening 
AOPT 
Material  axes  option  : 
EQ.0.0:  locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES,  and  then  rotated  about  the  shell  ele-
ment normal by the angle BETA. 
EQ.2.0:  globally orthotropic with material axes determined by
vectors  defined  below,  as  with  *DEFINE_COORDI-
C 
P 
VLCID 
FLAG 
*MAT_243 
DESCRIPTION
NATE_VECTOR. 
EQ.3.0:  locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by 
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the
element normal. 
LT.0.0:  the  absolute  value  of AOPT  is  a  coordinate system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available with the R3 release 
of Version 971 and later. 
C in Cowper-Symonds strain rate model 
p in Cowper-Symonds strain rate model, p = 0.0 for no strain rate 
effects 
Volume correction curve ID defining the relative volume change
(change in volume relative to the initial volume) as a function of
the effective plastic strain.  This is only used when nonzero.  See
Remark 1. 
Flag  for  interpretation  of  parameters.  If  FLAG = 1,  parameters 
AH,  BH,  and  CH  are  read  instead  of  R00,  R45,  and  R90.    See
Remark 4. 
XP, YP, ZP 
Coordinates of point p for AOPT = 1. 
A1, A2, A3 
Components of vector a for AOPT = 2. 
V1, V2, V3 
Components of vector v for AOPT = 3. 
D1, D2, D3 
Components of vector d for AOPT = 2. 
BETA 
Material angle in degrees for AOPT = 0 and 3, may be overridden 
on the element card, see *ELEMENT_SHELL_BETA. 
USRFAIL 
User defined failure flag  
USRFAIL.EQ.0:  no user subroutine is called 
USRFAIL.EQ.1:  user subroutine matusr_24 in dyn21.f is called
*MAT_HILL_90 
1.  The  effective  plastic  strain  used  in  this  model  is  defined  to  be  plastic  work 
equivalent.  A consequence of this is that for parameters defined as functions of 
effective  plastic  strain,  the  rolling  (00)  direction  should  be  used  as  reference 
direction.  For instance, the hardening curve for HR = 3 is the stress as function 
of strain for uniaxial tension in the rolling direction, VLCID curve should give 
the relative volume change as function of strain for uniaxial tension in the roll-
ing direction and load curve given by -E  should give the Young’s modulus as 
function  of  strain  for  uniaxial  tension  in  the  rolling  direction.    Optionally  the 
curve  can  be  substituted  for  a  table  defining  hardening  as  function  of  plastic 
strain rate (HR = 3) or temperature (HR = 8). 
2.  Exceptions from the rule above are curves defined as functions of plastic strain 
in the 45 and 90 directions, i.e., P1 and P2 for HR = 7 and negative R45 or R90.  
The hardening curves are here defined as measured stress as function of meas-
ured plastic strain for uniaxial tension in the direction of interest, i.e., as deter-
mined  from  experimental  testing  using  a  standard  procedure.    Moreover,  the 
curves  defining  the  R  values  are  as  function  of  the  measured  plastic  strain  for 
uniaxial  tension  in  the  direction  of  interest.    These  curves  are  transformed  in-
ternally  to  be  used  with  the  effective  stress  and  strain  properties  in  the  actual 
model.    The  effective  plastic  strain  does  not  coincide  with  the  plastic  strain 
components in other directions than the rolling direction and may be somewhat 
confusing to the user.  Therefore the von Mises work equivalent plastic strain is 
output  as  history  variable  #2  if  HR = 7  or  if  any  of  the  R-values  is  defined  as 
function of the plastic strain. 
3.  The R-values  in curves are defined as the ratio of instantaneous width change 
to instantaneous thickness change.  That is, assume that the width W and thick-
ness  T  are  measured  as  function  of  strain.    Then  the  corresponding  R-value  is 
given by: 
𝑅 =
𝑑𝑊
𝑑𝜀
𝑑𝑇
𝑑𝜀
/𝑊
/𝑇
4.  The anisotropic yield criterion Φ for plane stress is defined as: 
Φ = 𝐾1
𝑚 + 𝐾3𝐾2
(𝑚/2)−1 + 𝑐𝑚𝐾4
𝑚/2 = (1 + 𝑐𝑚 − 2𝑎 + 𝑏)𝜎𝑌
𝑚 
where 𝜎𝑌 is the yield stress and Ki = 1,4 are given by: 
𝐾1 = ∣𝜎𝑥 + 𝜎𝑦∣ 
𝐾2 = ∣𝜎𝑥
2 + 𝜎𝑦
2 ∣ 
2 + 2𝜎𝑥𝑦
𝐾3 = −2𝑎(𝜎𝑥
2 − 𝜎𝑦
2) + 𝑏(𝜎𝑥 − 𝜎𝑦)
𝐾4 = ∣(𝜎𝑥 − 𝜎𝑦)
2 ∣ 
+ 4𝜎𝑥𝑦
If FLAG = 0, the anisotropic material constants a, b, and c are obtained through 
R00, R45, and R90 using these 3 equations: 
1 + 2𝑅00 =
𝑐𝑚 − 𝑎 + {(𝑚 + 2)/2𝑚}𝑏
1 − 𝑎 + {(𝑚 − 2)/2𝑚}𝑏
1 + 2𝑅45 = 𝑐𝑚 
1 + 2𝑅90 =
𝑐𝑚 + 𝑎 + {(𝑚 + 2)/2𝑚}𝑏
1 + 𝑎 + {(𝑚 − 2)/2𝑚}𝑏
If FLAG = 1, material parameters a (AH), b (BH), and c (CH) are used directly. 
For  material  parameters  a,  b,  c,  and  m,  the  following  condition  has  to  be  ful-
filled, otherwise an error termination occurs: 
1 + 𝑐𝑚 − 2𝑎 + 𝑏    >    0 
Two  even  more  strict  conditions  should  ensure  convexity  of  the  yield  surface 
according to Hill (1990).  A warning message will be dumped if at least one of 
them is violated: 
𝑏 > −2
(𝑚
)−1
𝑐𝑚 
𝑏 > 𝑎2 − 𝑐𝑚 
The yield strength of the material can be expressed in terms of k and n: 
𝜎𝑌 = 𝑘𝜀𝑛 = 𝑘(𝜀𝑦𝑝 + 𝜀̅𝑝)
where 𝜀𝑦𝑝 is the elastic strain to yield and 𝜀̅𝑝 is the effective plastic strain (loga-
rithmic).    If  SIGY  is  set  to  zero,  the  strain  to  yield  if  found  by  solving  for  the 
intersection  of  the  linearly  elastic  loading  equation  with  the  strain  hardening 
equation: 
which gives the elastic strain at yield as: 
𝜎 = 𝐸𝜀 
𝜎 = 𝑘𝜀𝑛 
𝜀𝑦𝑝 = (
[ 1
]
𝑛−1
)
If SIGY yield is nonzero and greater than 0.02 then: 
𝜀𝑦𝑝 = (
𝜎𝑌
[1
𝑛]
)
The other available hardening models include the Voce equation given by 
𝜎Y(𝜀𝑝) = 𝑎 − 𝑏𝑒−𝑐𝜀𝑝,
the Gosh equation given by 
𝜎Y(𝜀𝑝) = 𝑘(𝜀0 + 𝜀𝑝)𝑛 − 𝑝, 
and finally the Hocket-Sherby equation given by 
𝜎Y(𝜀𝑝) = 𝑎 − 𝑏𝑒−𝑐𝜀𝑝
. 
For the Gosh hardening law, the interpretation of the variable SPI is the same, 
i.e.,  if  set  to  zero  the  strain  at yield  is  determined  implicitly  from  the  intersec-
tion of the strain hardening equation with the linear elastic equation. 
To  include  strain  rate  effects  in  the  model  we  multiply  the  yield  stress  by  a 
factor  depending  on  the  effective  plastic  strain  rate.    We  use  the  Cowper-
Symonds’ model, hence the yield stress can be written 
𝜎Y(𝜀𝑝, 𝜀̇𝑝) = 𝜎Y
⎡1 + (
⎢
⎣
𝑠  denotes the static yield stress, 𝐶 and 𝑝 are material parameters, 𝜀̇𝑝  is 
𝑠 (𝜀𝑝)
⎤ 
⎥
⎦
)
1/𝑝
𝜀̇𝑝
where 𝜎Y
the effective plastic strain rate. 
5.  A kinematic hardening model is implemented following the works of Chaboche 
and  Roussilier.    A  back  stress  α  is  introduced  such  that  the  effective  stress  is 
computed as 
𝜎eff = 𝜎eff(𝜎11 − 2𝛼11 − 𝛼22, 𝜎22 − 2𝛼22 − 𝛼11, 𝜎12 − 𝛼12) 
The back stress is the sum of up to four terms according to 
𝛼𝑖𝑗 = ∑ 𝛼𝑖𝑗
𝑘=1
and the evolution of each back stress component is as follows 
𝛿𝛼𝑖𝑗
𝑘 = 𝐶𝑘 (𝑎𝑘
𝑠𝑖𝑗
𝜎eff
− 𝛼𝑖𝑗
𝑘 ) 𝛿𝜀𝑝 
where 𝐶𝑘 and 𝑎𝑘 are material parameters,𝑠𝑖𝑗 is the deviatoric stress tensor, 𝜎eff is 
the effective stress and 𝜀𝑝 is the effective plastic strain.
*MAT_244 
This material model is developed for both shell and solid models.  It is mainly suited for 
hot stamping processes where phase transformations are crucial.  It has five phases and 
it is assumed that the blank is fully austenitized before cooling.  The basic constitutive 
model is based on the work done by P.  Akerstrom [2, 7]. 
Automatic switching  between cooling and heating of the blank is under development.  
To  activate  the  heating  algorithm,  set  HEAT = 1  or  2  and  add  the  appropriate  input 
Cards.  See the description of the HEAT parameter below.  HEAT = 0 as is the default 
activates  only  the  cooling  algorithm  and  no extra  cards  need  to  be  read  in.    Also  note 
that for HEAT = 0 you must check that the initial temperature of this material is above 
the  start  temperature  for  the  ferrite  transformation.    The  transformation  temperatures 
are echoed in the messag and in the d3hsp file.  
If HEAT > 0 the temperature that instantaneous transform all ferrite back to austenite is 
also echoed in the messag file.  If you want to heat up to 100% austenite you must let 
the specimen’s temperature exceed that temperature. 
Features Added in 2014: 
1.  Young’s  modulus  and  Poisson  ratio  can  now  be  given  as  temperature 
dependent load curves or by a table definition with a load curve for each phase.  
See Remark 8. 
2.  Latent heat can now be given for each phase.  See Remark 9. 
3.  Thermal expansion can now be given for each phase Remark 10. 
4.  Advanced  reaction  kinetic  modifications  include  the  ability  to  tailor  the  start 
temperatures and the activation energies.  The martensite start temperature can 
be  dependent  on  the  plastic  strain  and  triaxiality,  and  the  activation  energies 
can be scaled with the plastic strain as well. 
5.  Hardness  calculation  improved  when  tempering  is  active.    Improvements  are 
achieved in the bainite and martensite phases (experimental).  See Remark 11. 
NOTE:  For  this  material  “weight%”  means 
“ppm × 10-4”.
1 
Variable 
MID 
Type 
I 
2 
RO 
F 
3 
E 
F 
4 
PR 
F 
*MAT_UHS_STEEL 
5 
6 
7 
8 
TUNIT 
CRSH 
PHASE 
HEAT 
Defaults 
none 
none 
none 
none 
3600 
  Card 2 
1 
2 
3 
4 
5 
F 
I 
0 
6 
I 
0 
7 
Variable 
LCY1 
LCY2 
LCY3 
LCY4 
LCY5 
KFER 
KPER 
Type 
I 
I 
I 
I 
I 
F 
F 
I 
0 
8 
B 
F 
Defaults 
none 
none 
none 
none 
none 
0.0 
0.0 
0.0 
  Card 3 
Variable 
Type 
1 
C 
F 
2 
Co 
F 
3 
Mo 
F 
4 
Cr 
F 
5 
Ni 
F 
6 
Mn 
F 
7 
Si 
F 
8 
V 
F 
Defaults 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 4 
Variable 
Type 
1 
W 
F 
2 
Cu 
F 
3 
P 
F 
4 
Al 
F 
5 
As 
F 
6 
Ti 
F 
Defaults 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
7 
8 
CWM 
LCTRE 
I 
0 
I 
none
Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
THEXP1 
THEXP5 
LCTH1 
LCTH5 
TREF 
LAT1 
LAT5 
TABTH 
Type 
F 
F 
I 
I 
F 
F 
F 
I 
Defaults 
0.0 
0.0 
none 
none 
273.15 
0.0 
0.0 
none 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
QR2 
QR3 
QR4 
ALPHA 
GRAIN 
TOFFE 
TOFPE 
TOFBA 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Defaults 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 7 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PLMEM2  PLMEM3  PLMEM4  PLMEM5 
STRC 
STRP 
REACT 
TEMPER 
Type 
I 
F 
F 
F 
F 
F 
Defaults 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
I 
0 
I 
0 
Heat Card 1.  Additional Card for HEAT = 1. 
  Card 8 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
AUST 
FERR 
PEAR 
BAIN 
MART 
GRK 
GRQR 
TAU1 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
2.08E+8
Heat Card 2.  Additional Card for HEAT =1. 
  Card 9 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
GRA 
GRB 
EXPA 
EXPB 
GRCC 
GRCM 
HEATN 
TAU2 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
3.11 
7520. 
1.0 
1.0 
none 
none 
1.0 
4.806 
Reaction Card.  Addition card for REACT = 1. 
  Card 10 
Variable 
1 
FS 
Type 
F 
2 
PS 
F 
3 
BS 
F 
4 
5 
6 
7 
8 
MS 
MSIG 
LCEPS23 
LCEPS4 
LCEPS5 
F 
F 
I 
I 
I 
Default 
0.0 
0.0 
0.0 
0.0 
none 
none 
none 
none 
Tempering Card.  Additional card for TEMPR = 1. 
  Card 11 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCH4 
LCH5 
DTCRIT 
TSAMP 
Type 
Default 
I 
0 
I 
0 
F 
F 
0.0 
0.0
Computational Welding Mechanics Card.  Additional card for CWM  = 1. 
  Card 11 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TASTART   TAEND   TLSTART 
TLEND  
EGHOST 
PGHOST   AGHOST 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
VARIABLE 
DESCRIPTION  
BASELINE VALUE 
MID 
RO 
E 
Material  ID,  a  unique  number  has  to  be 
chosen. 
Material density
Youngs’ modulus: 
GT.0.0: constant value is used 
LT.0.0:  LCID  or  TABID.    Temperature 
dependent  Youngs’  modulus 
given  by  load  curve  ID = -E  or 
a  Table  ID = -E.    When  using  a 
table  to  describe  the  Youngs 
for 
modulus  see  Remark 8 
more information. 
7830 Kg/m3
100 GPa [1]
PR 
Poisson’s ratio: 
0.30 [1]
GT.0.0: constant value 
LT.0.0:  LCID or TABID: Temperature 
dependent  Poisson  ratio  given 
by load curve or table ID = -PR.  
The  table  input  is  described  in 
Remark 8. 
Number  of  time  units  per  hour.    Default 
is  seconds,  that  is  3600  time  units  per 
  It  is  used  only  for  hardness 
hour. 
calculations. 
TUNIT 
3600.
CRSH 
*MAT_UHS_STEEL 
DESCRIPTION  
BASELINE VALUE 
Switch  to  use  a  simple  and  fast  material 
model but with the actual phases active. 
EQ.0: The  original  model  where  phase 
transitions  are  active  and  trip  is 
used. 
EQ.1: A  simpler  and  faster  version.  
This  option 
is  mainly  when 
transferring  the  quenched  blank 
into  a  crash  analysis  where  all 
properties  from  the  cooling  are 
maintained.  This option must be 
*INTERFACE_-
used  with  a 
SPRINGBACK  keyword 
and 
should be used after a quenching 
analysis. 
EQ.2:  Same  as  0  but  trip  effect  is  not 
used. 
0 
0 
PHASE 
Switch  to  include  or  exclude  middle 
phases from the simulation. 
EQ.0: All phases active (default) 
EQ.1: pearlite and bainite excluded 
EQ.2: bainite excluded 
EQ.3: ferrite and pearlite excluded 
EQ.4: ferrite and bainite excluded 
EQ.5: exclude middle phases  
(only austenite → martensite)
VARIABLE 
DESCRIPTION  
BASELINE VALUE 
HEAT 
Switch to activate the heating algorithms 
EQ.0: Heating  is  not  activated.    That 
means  that  no  transformation  to 
Austenite is possible. 
EQ.1: Heating is activated: 
That 
means  that  only  transformation 
to Austenite is possible. 
EQ.2: Automatic  switching  between 
cooling  and  heating.    LS-DYNA 
checks  the  temperature  gradient 
and  calls  the  appropriate  algo-
rithms.  For example, this can be 
used  to  simulate  the  heat  affect-
ed zone during welding. 
LT.0:  Switch  between  cooling  and 
heating  is  defined  by  a  time  de-
pendent 
id 
  The  ordinate 
ABS(HEAT). 
should  be  1.0  when  heating  is 
applied and 0.0 if cooling is pref-
erable. 
load  curve  with 
LCY1 
Load  curve  or  Table  ID  for  austenite 
hardening. 
[5]
IF LCID 
input  yield  stress  versus  effective 
plastic strain. 
IF TABID.GT.0: 
2D table.  Input temperatures as table 
values  and  hardening  curves  as 
targets  for  those  temperatures   
IF TABID.LT.0: 
3D table.  Input temperatures as main 
table values and strain rates as values 
for  the  sub  tables,  and  hardening 
curves as targets for those strain rates.
VARIABLE 
DESCRIPTION  
BASELINE VALUE 
LCY2 
LCY3 
LCY4 
LCY5 
KFERR 
KPEAR 
B 
C 
Co 
Mo 
Cr 
Ni 
Mn 
Si 
V 
W 
Cu 
P 
Al 
As 
Ti 
Load  curve  ID  for  ferrite  hardening 
(stress versus eff.  pl.  str.) 
Load  curve  or  Table  ID  for  pearlite.    See 
LCY1 for description. 
Load  curve  or  Table  ID  for  bainite.    See 
LCY1 for description. 
Load  curve  or  Table  ID  for  martensite.  
See LCY1 for description. 
Correction  factor  for  boron  in  the  ferrite 
reaction. 
Correction factor for boron in the pearlite 
reaction. 
Boron [weight %]
Carbon [weight %]
Cobolt [weight %]
Molybdenum [weight %]
Chromium [weight %]
Nickel [weight %]
Manganese [weight %]
Silicon [weight %]
Vanadium [weight %]
Tungsten [weight %]
copper [weight %]
Phosphorous [weight %]
Aluminium [weight %]
Arsenic [weight %]
Titanium [weight %]
1.9 × 105 [2] 
3.1 × 103 [2] 
0.003 [2, 4]
0.23 [2, 4]
0.0 [2, 4]
0.0 [2, 4]
0.21 [2, 4]
0.0 [2, 4]
1.25 [2, 4]
0.29 [2, 4]
0.0 [2, 4]
0.0
0.0
0.013
0.0
0.0
0.0
VARIABLE 
CWM 
LCTRE 
THEXP1 
THEXP5 
LCTH1 
LCTH5 
TREF 
LAT1 
DESCRIPTION  
BASELINE VALUE 
for 
Flag 
computational  welding 
mechanics  input.    One  additional  input 
card is read. 
EQ.1.0: Active  
EQ.0.0: Inactive 
Load  curve  for  transformation  induced 
for  more 
strains. 
information. 
  See  Remark  13 
Coefficient  of 
austenite 
Coefficient  of 
martensite 
thermal  expansion 
in 
25.1 × 10−6 1/K [7] 
thermal  expansion 
in 
11.1 × 10−6 1/K [7] 
0 
0 
293.15
590 × 106 J/m3 [2] 
the 
Load  curve 
coefficient for austenite: 
for 
thermal  expansion 
LT.0.0:  curve ID = -LA and TREF is used as 
reference temperature 
GT.0.0:  curve ID = LA 
Load  curve 
coefficient for martensite: 
the 
for 
thermal  expansion 
LT.0.0:  curve ID = -LA and TREF is used as 
reference temperature 
GT.0.0:  curve ID = LA 
temperature 
thermal 
Reference 
expansion.  Used if and only if LA.LT.0.0 
or/and LM.LT.0.0 
for 
Latent  heat  for  the  decomposition  of 
austenite into ferrite, pearlite and bainite. 
GT.0.0: Constant value 
LT.0.0:  Curve  ID  or  Table  ID.    See 
infor-
for  more 
Remark 9 
mation.
LAT5 
TABTH 
QR2 
QR3 
QR4 
ALPHA 
GRAIN 
TOFFE 
2-1220 (EOS) 
DESCRIPTION  
Latent  heat  for  the  decomposition  of 
austenite into martensite. 
GT.0.0: Constant value 
LT.0.0:  Curve ID: Note  that  LAT  5  is 
ignored if a Table ID is used in 
LAT1. 
for 
thermal  expansion 
Table  definition 
coefficient.    With  this  option  active  THEXP1, 
THEXP2, LCTH1 and LCTH5 are ignored.  See 
Remark 10. 
GT.0:  A  table  for  instantaneous  thermal 
expansion (TREF is ignored). 
LT.0:  A  table  with  thermal  expansion  with 
reference to TREF. 
energy  divided  by 
Activation 
the 
universal  gas  constant  for  the  diffusion 
reaction  of  the  austenite-ferrite  reaction: 
Q2/R.  R = 8.314472 [J/mol K]. 
energy  divided  by 
the 
Activation 
universal  gas  constant  for  the  diffusion 
reaction 
austenite-pearlite 
the 
reaction: Q3/R.  R = 8.314472 [J/mol K]. 
for 
energy  divided  by 
Activation 
the 
universal  gas  constant  for  the  diffusion 
reaction for the austenite-bainite reaction: 
Q4/R.  R = 8.314472 [J/mol K]. 
for 
Material  constant 
the  martensite 
phase.    A  value  of  0.011  means  that  90% 
of  the  available  austenite  is  transformed 
into  martensite  at  210  degrees  below  the 
martensite start temperature ,  whereas  a  value  of 
0.033 means a 99.9% transformation. 
ASTM  grain  size  number  for  austenite, 
usually a number between 7 and 11. 
Number  of  degrees  that  the  ferrite  is 
bleeding over into the pearlite reaction. 
*MAT_UHS_STEEL 
BASELINE VALUE 
640 × 106 J/m3 [2] 
10324 K [3] =
(23000 cal/mole) × 
(4.184 J/cal) / 
(8.314 J/mole/K) 
13432.  K [3]
15068.  K [3]
0.011
6.8
VARIABLE 
DESCRIPTION  
BASELINE VALUE 
TOFPE 
TOFBA 
PLMEM2 
PLMEM3 
PLMEM4 
PLMEM5 
Number  of  degrees  that  the  pearlite  is 
bleeding over into the bainite reaction 
Number  of  degrees  that  the  bainite  is 
bleeding  over 
the  martensite 
into 
reaction. 
Memory  coefficient  for  the  plastic  strain 
that is carried over from the austenite.  A 
value  of  1  means  that  all  plastic  strains 
from austenite is transferred to the ferrite 
phase  and  a  value  of  0  means  that 
nothing is transferred. 
Same  as  PLMEM2  but  between  austenite 
and pearlite. 
Same  as  PLMEM2  but  between  austenite 
and bainite. 
Same  as  PLMEM3  but  between  austenite 
and martensite. 
STRC 
Effective strain rate parameter C. 
STRC.LT.0.0:  load curve id = -STRC  
STRC.GT.0.0:  constant value 
STRC.EQ.0.0:  strain rate NOT active 
STRP 
Effective strain rate parameter P. 
STRP.LT.0.0:  load curve id = -STRP 
STRP.GT.0.0: constant value 
STRP.EQ.0.0: strain rate NOT active 
REACT 
Flag for advanced reaction kinetics input.  
One additional input card is read. 
EQ.1.0: Active  
EQ.0.0: Inactive 
0.0
0.0
0.0
0.0
0.0
0.0
0.0
0.0
0.0
TEMPER 
AUST 
FERR 
PEAR 
BAIN 
MART 
GRK 
GRQR 
TAU1 
GRA 
GRB 
EXPA 
EXPB 
GRCC 
*MAT_UHS_STEEL 
DESCRIPTION  
BASELINE VALUE 
Flag for tempering input.  One additional 
input card is read. 
EQ.1.0: Active 
EQ.0.0: Inactive 
If  a  heating  process  is  initiated  at  t = 0 
this  parameters  sets  the  initial  amount  of 
austenite  in  the  blank.    If  heating  is 
activated at t > 0 during a simulation this 
value is ignored.  Note that, 
AUST + FERR + PEAR + BAIN
+ MART = 1.0 
See AUST for description
See AUST for description
See AUST for description
See AUST for description
Growth parameter k (μm2/sec)
Grain  growth  activation  energy  (J/mol) 
divided  by  the  universal  gas  constant.  
Q/R where R = 8.314472 (J/mol K) 
Empirical  grain  growth  parameter  𝑐1
describing the function τ(T) 
Grain growth parameter A
Grain  growth  parameter  B.    A  table  of 
recommended values of GRA and GRB is 
included in Remark 7. 
Grain growth parameter a
Grain growth parameter b
Grain  growth  parameter  with 
the 
concentration  of  non-metals  in  the  blank, 
weight% of C or N  
0.0
0.0
0.0
0.0
0.0
0.0
1011 [9] 
3 × 104 [9] 
2.08 × 108 [9] 
 [9]
 [9]
1.0 [9]
1.0 [9]
[9]
VARIABLE 
GRCM 
HEATN 
TAU2 
DESCRIPTION  
BASELINE VALUE 
Grain  growth  parameter  with 
the 
concentration  of  metals  in  the  blank, 
lowest weight% of Cr, V, Nb, Ti, Al. 
[9]
Grain  growth  parameter  n 
austenite formation 
for 
the 
1.0 [9]
Empirical  grain  growth  parameter  𝑐2
describing the function τ(T) 
4.806 [9]
FS 
Manual start temperature Ferrite  
GT.0.0:  Same 
temperature 
heating and cooling.  
is  used 
for 
LT.0.0:  Curve ID: 
Different 
start 
temperatures  for  cooling  and  heat-
ing  given  by  load  curve  ID = -FS.  
First ordinate value is used for cool-
ing, last ordinate value for heating. 
PS 
BS 
MS 
MSIG 
LCEPS23 
Manual start temperature Pearlite.  See FS 
for description. 
Manual start temperature Bainite.  See FS 
for description. 
Manual start temperature Martensite.  See 
FS for description. 
Describes  the  increase  of  martensite  start 
temperature  for  cooling  due  to  applied 
stress. 
LT.0: Load Curve ID describes MSIG as 
a  function  of  triaxiality  (pressure 
/ effective stress). 
MS* = MS + MSIG × 𝜎eff 
Load  Curve  ID  dependent  on  plastic 
strain  that  scales  the  activation  energy 
QR2 and QR3. 
QRx = Qx × CEPS23(𝜀pl) / R
BASELINE VALUE 
Load  Curve  ID  dependent  on  plastic 
strain  that  scales  the  activation  energy 
QR4. 
QR4 = Q4 × LCEPS4(𝜀pl) / R 
ID  which  describe 
the  martensite 
the 
Load  Curve 
increase 
start 
of 
temperature  for  cooling  as  a  function  of 
plastic strain. 
MS* = MS + MSIG × 𝜎eff + LCEPS5(𝜀pl) 
Load  curve  ID  of  Vicker  hardness  vs.  
hardness 
temperature 
calculation. 
Bainite 
for 
Load  curve  ID  of  Vicker  hardness  vs.  
for  Martensite  hardness 
temperature 
calculation. 
Critical  cooling  rate  to  detect  holding 
phase. 
Sampling  interval  for  temperature  rate 
monitoring to detect the holding phase 
Annealing temperature start
Annealing temperature end
Birth temperature start
Young’s  modulus 
material 
for  ghost  (quiet) 
Poisson’s ratio for ghost (quiet) material
Thermal  expansion  coefficient  for  ghost 
(quiet) material 
*MAT_244 
VARIABLE 
LCEPS4 
LCEPS5 
LCH4 
LCH5 
DTCRIT 
TSAMP 
TASTART 
TAEND 
TLSTART 
EGHOST 
PGHOST 
AGHOST 
Discussion: 
The  phase  distribution  during  cooling  is  calculated  by  solving  the  following  rate 
equation for each phase transition 
𝑋̇𝑘 = 𝑔𝑘(𝐺, 𝐶, 𝑇𝑘, 𝑄𝑘)𝑓𝑘(𝑋𝑘),
𝑘 = 2,3,4
where  𝑔𝑘  is  a  function,  taken  from  Li  et  al.,    dependent  on  the  grain  number  G,  the 
chemical composition C, the temperature T and the activation energy Q.  Moreover, the 
function f is dependent on the actual phase 𝑋𝑘 = 𝑥𝑘/𝑥eq 
0.4(𝑋𝑘−1)(1 − 𝑋𝑘)0.4𝑋𝑘,
The true amount of martensite, i.e., 𝑘 = 5, is modelled by using the true amount of the 
austenite left after the bainite phase: 
𝑓𝑘(𝑋𝑘) = 𝑋𝑘
𝑘 = 2,3,4 
𝑥5 = 𝑥1[1 − 𝑒−𝛼(MS−𝑇)], 
where 𝑥1 is the true amount of austenite left for the reaction, 𝛼 is a material dependent 
constant and MS is the start temperature of the martensite reaction. 
The start temperatures are automatically calculated based on the composition: 
1.  Ferrite, 
 FS = 1185 − 203 × √C − 15.2 × Ni + 44.7 × Si + 104 × V + 31.5 × Mo + 13.1 × W
− 30 × Mn − 11 × Cr − 20 × Cu + 700 × P + 400 × Al + 120 × As
+ 400 × Ti 
2.  Pearlite, 
PS = 996 − 10.7 × Mn − 16.9 × Ni + 29 × Si + 16.9 × Cr + 290 × As + 6.4 × W 
3.  Bainite, 
BS = 910 − 58 × C − 35 × Mn − 15 × Ni − 34 × Cr − 41 × Mo 
4.  Martensite, 
MS = 812 − 423 × C − 30.4 × Mn − 17.7 × Ni − 12.1 × Cr − 7.5 × Mo + 10 × Co
− 7.5 × Si 
where the element weight values are input on Cards 2 through 4. 
The  automatic  start  temperatures  are  printed  to  the  messag  file  and  if  they  are  not 
accurate enough you can manually set them in the input deck (must be set in absolute 
temperature,  Kelvin).    If  HEAT > 0,  the  temperature  FSnc  (ferrite  without  C)  is  also 
echoed.  If the specimen exceeds that temperature all ferrite that is left is instantaneous 
transformed to austenite. 
Remarks: 
1.  History Variables.  History variables 1 through 8 include the different phases, 
the  Vickers  hardness,  the  yield  stress  and  the  ASTM  grain  size  number.    Set 
NEIPS = 8 (shells) or NEIPH = 8 (solids)  on *DATABASE_EXTENT_BINARY.
History 
Variable 
1 
2 
3 
4 
5 
6 
7 
8 
Description 
Amount austenite 
Amount ferrite 
Amount pearlite 
Amount bainite 
Amount martensite 
Vickers hardness 
Yield stress 
grain 
size 
ASTM 
number  (a  low  value 
means large grains and 
vice versa) 
2.  Excluding  Phases.    To  exclude  a  phase  from  the  simulation,  set  the  PHASE 
parameter accordingly. 
3.  STRC and STRP.  Note that both strain rate parameters must be set to include 
the  effect.    It  is  possible  to  use  a  temperature  dependent  load  curve  for  both 
parameters simultaneously or for one parameter keeping the other constant. 
4.  TUNIT.    TUNIT  is  time  units  per  hour  and  is  only  used  for  calculating  the 
Vicker Hardness, as default it is assumed that the time unit is seconds.  If other 
time  unit  is  used,  for  example  milliseconds,  then  TUNIT  must  be  changed  to 
TUNIT = 3.6 × 106 
5.  TSF.    The  thermal  speedup  factor  TSF of  *CONTROL_THERMAL_SOLVER  is 
used to scale reaction kinetics and hardness calculations in this material model.  
On  the  other  hand,  strain  rate  dependent  properties   are not scaled by TSF. 
6.  CRSH.    With  the  CRSH = 1  option  it  is  now  possible  to  transfer  the  material 
properties from a hot stamping simulation (CRSH = 0) into another simulation.  
The CRSH = 1 option reads a dynain file from a simulation with CRSH = 0 and 
keeps  all  the  history  variables  (austenite,  ferrite,  pearlite,  bainite,  martensite, 
etc)  constant.    This  will  allow  steels  with  inhomogeneous  strength  to  be  ana-
lysed in, for example, a crash simulation.  The speed with the CRSH = 1 option 
is  comparable  with  *MAT_024.    Note  that  for  keeping  the  speed  the  tempera-
ture  used  in  the  CRSH  simulation  should  be  constant  and  the  thermal  solver 
should be inactive.
7.  HEAT.    When  HEAT  is  activated  the  re-austenitization  and  grain  growth 
algorithms are also activated.  The grain growth is activated when the tempera-
ture exceeds a threshold value that is given by  
𝑇 =
𝐴 − log10[(GRCM)𝑎(GRCC)𝑏]
and the rate equation for the grain growth is, 
𝑔̇ =
𝑅𝑇. 
−
2𝑔
The rate equation for the phase re-austenitization is given in Oddy (1996) and is 
here mirrored 
𝑥̇𝑎 = 𝑛 [ln (
𝑥𝑒𝑢
𝑥𝑒𝑢 − 𝑥𝑎
𝑛−1
)]
[
𝑥𝑒𝑢 − 𝑥𝑎
𝜏(𝑇)
] 
where n is the parameter HEATN.  The temperature dependent function 𝜏(𝑇) is 
given  from  Oddy  as  𝜏(𝑇) = 𝑐1(𝑇 − 𝑇𝑠)𝑐2.  The  empirical  parameters  𝑐1  and  𝑐2 
are calibrated in Oddy to 2.06 × 108 and 4.806 respectively.  Note that 𝜏 above 
given in seconds. 
Recommended values for GRA and GRB are given in the following table. 
Compound 
Metal 
Non-metal 
GRA 
Cr23C6 
V4C3 
TiC 
NbC 
Mo2C 
Nb(CN) 
VN 
AlN 
NbN 
TiN 
Cr 
V 
Ti 
Nb 
Mo 
Nb 
V 
Al 
Nb 
Ti 
C 
C0.75 
C 
C0.7 
C 
(CN) 
N 
N 
N 
N 
5.90 
5.36 
2.75 
3.11 
5.0 
2.26 
3.46 + 0.12%Mn
1.03 
4.04 
0.32 
GRB 
7375 
8000 
7000 
7520 
7375 
6770 
8330 
6770 
10230 
8000 
8.  Using  the  Table  Capability  for  Temperature  Dependence  of  Young’s 
Modulus.    Use  *DEFINE_TABLE_2D  and  set  the  abscissa  value  equal  to  1  for 
the  austenite  YM-curve,  equal  to  2  for  the  ferrite  YM-curve,  equal  to  3  for  the 
pearlite YM curve, equal to 4 for the bainite YM-curve and finally equal to 5 for 
the martensite YM-curve.  If you use the PHASE option you only need to define
the curves for the included phases, but you can define all five.  LS-DYNA uses 
the number 1-5 to get the right curve for the right phase.  The total YM is calcu-
lated  by  a  linear  mixture  law:  YM = YM1 × PHASE1 + ⋯ + YM5 × PHASE5.  
For example: 
*DEFINE_TABLE_2D 
$ The number before curve id:s define which phase the curve 
$ will be applied to.  1 = Austenite, 2 = Ferrite, 3 = Pearlite, 
$ 4 = Bainite and 5 = Martensite.  
      1000       0.0       0.0 
                 1.0                 100 
                 2.0                 200 
                 3.0                 300 
                 4.0                 400 
                 5.0                 500 
$ 
$ Define curves 100 - 500 
*DEFINE_CURVE 
$ Austenite Temp (K) - YM-Curve (MPa) 
       100         0       1.0       1.0 
              1300.0              50.E+3 
               223.0             210.E+3 
9.  Using  the  Table  Capability  for  Latent  Heat.    When  using  a  table  ID  for  the 
latent heat (LAT1) you can describe all phase transition individually.  Use *DE-
FINE_TABLE_2D and set the abscissa values to the corresponding phase transi-
tion number.  That is, 2 for the austenite to ferrite, 3 for the austenite to pearlite, 
4  for  the  austenite  to  bainite  and  5  for  the  austenite  to  martensite.    Remark  8 
demonstrates the form a correct table definition.  If a curve is missing, the cor-
responding latent heat for that transition will be set to zero.  Also, when a table 
is used the LAT2 is ignored.  If HEAT > 0 you also have the option to include 
latent heat for the transition back to Austenite.  This latent heat curve is marked 
as 1 in the table definition of LAT1. 
10.  Using  the  Table  Capability  for  Thermal  Expansion.   When  using  a  table  ID 
for the thermal expansion you can specify the expansion characteristics for each 
phase.  That is, you can have a curve for each of the 5 phases (austenite, ferrite, 
pearlite, bainite, and martensite).  The input is identical to the above table defi-
nitions.    The  table  must  have  the  abscissa  values  between  1  and  5  where  the 
number correspond to phase 1 to 5.  To exclude one phase from influencing the 
thermal expansion you simply input a curve that is zero for that phase or even 
easier,  exclude  that  phase  number  in  the  table  definition.    For  example,  to  ex-
clude the bainite phase you only define the table with curves for the indices 1, 2, 
3 and 5. 
11.  TEMPER.    Tempering  is  activated  by  setting  TEMPER  to  1.    When  active  the 
default  hardness  calculation  for  bainite  and  martensite  is  altered  to  use  an  in-
cremental update formula.  The total hardness is given by ∑ HV𝑖 × 𝑥𝑖
 .  When 
holding phases are detected the hardness for Bainite and Martensite is updated 
according to 
𝑖=1
HV4
𝑛+1 =
HV5
𝑛+1 =
𝑥4
𝑛+1 HV4
𝑥4
𝑥5
𝑛+1 HV5
𝑥5
𝑛 +
𝑛 +
∆𝑥4
𝑛+1 ℎ4(𝑇),
𝑥4
∆𝑥5
𝑛+1 ℎ5(𝑇),
𝑥5
∆𝑥4 = 𝑥4
𝑛+1 − 𝑥4
𝑛 
∆𝑥5 = 𝑥5
𝑛+1 − 𝑥5
𝑛 
We detect the holding phase for Bainite and Martensite when the temperature 
is  in  the  appropriate  range  and  if  average  temperature  rate  is  below  DTCRIT.  
𝑛 +
The  average  temperature  rate  is  calculated  as 
𝑛 + ∆𝑡. The average temperature and time are updated until 
∣𝑇̇∣∆𝑡 and 𝑡tresh
𝑡tresh ≥ 𝑡samp. 
  where  the  𝑇tresh
𝑛+1 = 𝑇tresh
𝑛+1 = 𝑡tresh
𝑇tresh
𝑡tresh
12.  CWM  (Welding).    When  computational  welding  mechanics  is  activated  with 
CWM = 1 the material can be defined to be initially in a quiet state.  In this state 
the material (often referred to as ghost material) has thermo-mechanical proper-
ties defined by an additional card.  The material is activated when the tempera-
ture reaches the birth temperature.  See MAT_CWM (MAT_270) for a detailed 
description. 
13.  LCTRE  (Transformation  Induced  Strains).    Transformation  induced  strains 
can  be  included  with  a  load  curve  LCTRE  as  a  function  of  temperature.    The 
load curve represents the difference between the hard phases and the austenite 
phase  in  the  dilatometer  curves.    Therefore,  positive  curve  values  result  in  a 
negative transformation strain for austenitization and a positive transformation 
strain for the phase transformation from austenite to one of the hard phases.  
References: 
1.  Numisheet  2008  Proceedings,  The  Numisheet  2008  Benchmark Study,  Chapter 
3,  Benchmark  3,  Continuous  Press  Hardening,  Interlaken,  Switzerland,  Sept.  
2008. 
2.  P.    Akerstrom  and  M.    Oldenburg,  “Austenite  Decomposition  During  Press 
hardening of a Boron Steel – Computer Simulation and Test”, Journal of Mate-
rial processing technology, 174 (2006), pp399-406. 
3.  M.V  Li,  D.V  Niebuhr,  L.L  Meekisho  and  D.G  Atteridge,  “A  Computatinal 
model  for  te  prediction  of  steel  hardenability”,  Metallurgical  and  materials 
transactions B, 29B, 661-672, 1998. 
4.  D.F.  Watt, “An Algorithm for Modelling Microstructural Development in Weld 
heat-Affected Zones (Part A) Reaction Kinetics”, Acta metal.  Vol.  36., No.  11, 
pp.  3029-3035, 1988.
5.  ThyssenKrupp  Steel,  “Hot  Press  hardening  Manganese-boron  Steels  MBW”, 
product information Manganese-boron Steels, Sept.  2008. 
6.  Malek  Naderi,  “Hot  Stamping  of  Ultra  High  Strength  Steels”,  Doctor  of 
Engineering Dissertation, Technical University Aachen, Germany, 2007. 
7.  P.    Akerstrom,  “Numerical  Implementation  of  a  Constitutive  model  for 
Simulation of Hot Stamping”, Division of Solid Mechanics, Lulea University of 
technology, Sweden. 
8.  Malek Naderi, “A numerical and Experimental Investigation into Hot Stamping 
of Boron Alloyed Heat treated Steels”, Steel research Int.  79 (2008) No.  2. 
9.  A.S.    Oddy,  J.M.J.    McDill  and  L.    Karlsson,  “Microstructural  predictions 
including  arbitrary  thermal  histories,  reaustenitization  and  carbon  segregation 
effects” (1996). 
Boron steel composition from the literature: 
Element 
HAZ code 
Akerstrom (2) 
Naderi (8) 
ThyssenKrupp(4)
(max amount) 
B 
C 
Co 
Mo 
Cr 
Ni 
Mn 
Si 
V 
W 
Cu 
P 
Al 
As 
Ti 
S 
0.168 
0.036 
0.255 
0.015 
1.497 
0.473 
0.026 
0.025 
0.012 
0.020 
0.003 
0.23 
0.211 
1.25 
0.29 
0.003 
0.230 
0.160 
1.18 
0.220 
0.005 
0.250 
0.250 
0.250 
1.40 
0.400 
0.013 
0.015 
0.025 
0.003 
0.040 
0.001 
0.05 
0.010
*MAT_PML_OPTIONTROPIC_ELASTIC 
This  is  Material  Type  245.    This  is  a  perfectly-matched  layer  (PML)  material  for 
orthotropic  or  anisotropic  media,  to  be  used  in  a  wave-absorbing  layer  adjacent  to  an 
orthotropic/anisotropic  material  (*MAT_{OPTION}TROPIC_ELASTIC)  in  order  to 
simulate wave propagation in an unbounded ortho/anisotropic medium.  
This material is a variant of MAT_PML_ELASTIC (MAT_230) and is available only for 
solid  8-node  bricks 
follow 
*MAT_{OPTION}TROPIC_ELASTIC as shown below.  See the variable descriptions and 
Remarks section of *MAT_{OPTION}TROPIC_ELASTIC (*MAT_002) for further details.  
input  cards  exactly 
type  2). 
(element 
  The 
Available options include: 
ORTHO 
ANISO 
such that the keyword cards appear: 
*MAT_PML_ORTHOTROPIC_ELASTIC or MAT_245 
(4 cards follow) 
*MAT_PML_ANISOTROPIC_ELASTIC or MAT_245_ANISO 
(5 cards follow) 
Orthotropic Card 1.  Card 1 format used for ORTHO keyword option. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
EA 
F 
4 
EB 
F 
5 
EC 
F 
6 
7 
8 
PRBA 
PRCA 
PRCB 
F 
F 
F 
Orthotropic Card 2.  Card 2 format used for ORTHO keyword option. 
  Card 2 
1 
2 
3 
4 
Variable 
GAB 
GBC 
GCA 
AOPT 
Type 
F 
F 
F 
F 
5 
G 
F 
6 
7 
8 
SIGF
Anisotropic Card 1.  Card 1 format used for ANISO keyword option. 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
4 
5 
6 
7 
8 
C11 
C12 
C22 
C13 
C23 
C33 
Type 
A8 
F 
F 
F 
F 
F 
F 
F 
Anisotropic Card 2.  Card 2 format used for ANISO keyword option. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
C14 
C24 
C34 
C44 
C15 
C25 
C35 
C45 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Anisotropic Card 3.  Card 3 format used for ANISO keyword option. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
C55 
C16 
C26 
C36 
C46 
C56 
C66 
AOPT 
Type 
F 
F 
F 
F 
F 
F 
  Card 4 
Variable 
1 
XP 
Type 
F 
  Card 5 
Variable 
1 
V1 
Type 
F 
2 
YP 
F 
2 
V2 
F 
3 
ZP 
F 
3 
V3 
F 
4 
A1 
F 
4 
D1 
F 
5 
A2 
F 
5 
D2 
F 
6 
A3 
F 
6 
D3 
F 
F 
7 
MACF 
I 
7 
F 
8 
8 
BETA 
REF 
F
Remarks: 
1.  A layer of this material may be placed at a boundary of a bounded domain to 
simulate unboundedness of the domain at that boundary: the layer absorbs and 
attenuates  waves  propagating  outward  from  the  domain,  without  any  signifi-
cant  reflection  of  the  waves  back  into  the  bounded  domain.    The  layer  cannot 
support any static displacement.  
2. 
It is assumed the material in the bounded domain near the layer is, or behaves 
like,  a    linear  ortho/anisotropic  material.    The  material  properties  of  the  layer 
should be set to the corresponding properties of this material.  
3.  The layer should form a cuboid box around the bounded domain, with the axes 
of the box aligned with the coordinate axes.  Various faces of this  box may be 
open,  as  required  by  the  geometry  of  the  problem,  e.g.,  for  a  half-space  prob-
lem, the “top” of the box should be open. 
4. 
Internally, LS-DYNA will partition the entire PML into regions which form the 
“faces”,  “edges”  and  “corners”  of  the  above  cuboid  box,  and  generate  a  new 
material for each region.  This partitioning will be visible in the d3plot file.  The 
user may safely ignore this partitioning. 
5.  The  layer  should  have  5 - 10  elements  through  its  depth.    Typically,  5 - 6 
elements  are  sufficient  if  the  excitation  source  is  reasonably  distant  from  the 
layer, and 8 - 10 elements if it is close.  The size of the elements should be simi-
lar  to  that  of  elements  in  the  bounded  domain  near  the  layer,  and  should  be 
small  enough  to  sufficiently  discretize  all  significant  wavelengths  in  the  prob-
lem. 
6.  The nodes on the outer boundary of the layer should be fully constrained.  
7.  The stress and strain values reported by this material do not have any physical 
significance.
*MAT_PML_NULL 
This  is  Material  Type  246.    This  is  a  perfectly-matched  layer  (PML)  material  with  a 
pressure  fluid  constitutive  law  computed  using  an  equation  of  state,  to  be  used  in  a 
wave-absorbing layer adjacent to a fluid material (*MAT_NULL with an EOS) in order 
to simulate wave propagation in an unbounded fluid medium.  Only *EOS_LINEAR_-
POLYNOMIAL  and  *EOS_GRUNEISEN  are  allowed  with  this  material.    See  the 
Remarks  section  of  *MAT_NULL  (*MAT_009)  for  further  details.    Accurate  results  are 
to be expected only for the case where the EOS presents a linear relationship between 
the pressure and volumetric strain.  
This material is a variant of MAT_PML_ELASTIC (MAT_230) and is available only for 
solid 8-node bricks (element type 2).  
4 
5 
6 
7 
8 
Card 
1 
Variable 
MID 
2 
RO 
3 
MU 
Type 
A8 
F 
F 
Default 
none 
none 
0.0 
  VARIABLE   
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Dynamic viscosity coefficient 
MID 
RO 
MU 
Remarks: 
1.  A layer of this material may be placed at a boundary of a bounded domain to 
simulate unboundedness of the domain at that boundary: the layer absorbs and 
attenuates  waves  propagating  outward  from  the  domain,  without  any  signifi-
cant  reflection  of  the  waves  back  into  the  bounded  domain.    The  layer  cannot 
support any static displacement.  
2. 
It is assumed the material in the bounded domain near the layer is, or behaves 
like, an linear fluid material.  The material properties of the layer should be set 
to the corresponding properties of this material.
3.  The layer should form a cuboid box around the bounded domain, with the axes 
of the box aligned with the coordinate axes.  Various faces of this  box may be 
open,  as  required  by  the  geometry  of  the  problem,  e.g.,  for  a  half-space  prob-
lem, the “top” of the box should be open. 
4. 
Internally, LS-DYNA will partition the entire PML into regions which form the 
“faces”,  “edges”  and  “corners”  of  the  above  cuboid  box,  and  generate  a  new 
material for each region.  This partitioning will be visible in the d3plot file.  The 
user may safely ignore this partitioning. 
5.  The layer should have 5-10 elements through its depth.  Typically, 5-6 elements 
are sufficient if the excitation source is reasonably distant from the layer, and 8-
10 elements if it is close.  The size of the elements should be  similar to that of 
elements in the bounded domain near the layer, and should be small enough to 
sufficiently discretize all significant wavelengths in the problem. 
6.  The nodes on the outer boundary of the layer should be fully constrained.  
7.  The stress and strain values reported by this material do not have any physical 
significance.
*MAT_PHS_BMW 
This  is  Material  Type  248.    This  model  is  intended  for  hot  stamping  processes  with 
phase  transformation  effects.    It  is  available  for  shell  elements  only  and  is  based  on 
Material Type 244 (*MAT_UHS_STEEL).  As compared with Material Type 244 Material 
Type 248 features: 
1. 
2. 
3. 
a more flexible choice of evolution parameters, 
an approach for transformation induced strains, 
and a more accurate density calculation of individual phases. 
Thus  the  metal  physical  effects  can  be  taken  into  account  calculating  the  volume 
fractions  of  ferrite,  pearlite,  bainite  and  martensite  for  fast  supercooling  as  well  as  for 
slow  cooling  conditions.    Furthermore,  this  material  model  features  cooling-rate 
dependence  for  several  of  its  more  crucial  material  parameters  in  order  to  accurately 
calculate  the  Time-Temperature-Transformation  diagram  dynamically.    A  detailed 
description can be found in Hippchen et al.  [2013] and Hippchen [2014]. 
NOTE 1:  For this material “weight%” means 
“ppm × 10-4”. 
NOTE 2:  For  this  material  the  phase  frac-
tions  are  calculated  in  volume  per-
cent (vol%). 
  Card 1 
1 
Variable 
MID 
Type 
I 
2 
RO 
F 
3 
E 
F 
4 
PR 
F 
Defaults 
none 
none 
none 
none 
3600 
5 
6 
7 
8 
TUNIT 
TRIP 
PHASE 
HEAT 
F 
I 
0 
I 
0 
I
Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCY1 
LCY2 
LCY3 
LCY4 
LCY5 
C_F 
C_P 
C_B 
Type 
I 
I 
I 
I 
I 
F 
F 
F 
Defaults 
none 
none 
none 
none 
none 
0.0 
0.0 
0.0 
  Card 3 
Variable 
Type 
1 
C 
F 
2 
Co 
F 
3 
Mo 
F 
4 
Cr 
F 
5 
Ni 
F 
6 
Mn 
F 
7 
Si 
F 
8 
V 
F 
Defaults 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 4 
Variable 
Type 
1 
W 
F 
2 
Cu 
F 
3 
P 
F 
4 
Al 
F 
5 
As 
F 
6 
Ti 
F 
7 
B 
F 
8 
Defaults 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Defaults 
TABRHO 
TREF 
LAT1 
LAT5 
TABTH 
I 
F 
F 
F 
I 
none 
none 
0.0 
0.0 
none
Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
QR2 
QR3 
QR4 
ALPHA 
GRAIN 
TOFFE 
TOFPE 
TOFBA 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Defaults 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 7 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PLMEM2  PLMEM3  PLMEM4  PLMEM5 
STRC 
STRP 
Type 
F 
F 
F 
F 
F 
F 
Defaults 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 8 
Variable 
1 
FS 
Type 
F 
2 
PS 
F 
3 
BS 
F 
4 
5 
6 
7 
8 
MS 
MSIG 
LCEPS23 
LCEPS4 
LCEPS5 
F 
F 
I 
I 
I 
Defaults 
0.0 
0.0 
0.0 
0.0 
none 
none 
none 
none 
  Card 9 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCH4 
LCH5 
DTCRIT 
TSAMP 
ISLC 
IEXTRA 
Type 
Defaults 
I 
0 
I 
0 
F 
F 
0.0 
0.0 
I 
0 
I
Card 10 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ALPH_M 
N_M 
PHI_M 
PSI_M 
OMG_F 
PHI_F 
PSI_F 
CR_F 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Defaults 
0.0428 
0.191 
0.382 
2.421 
0.41 
0.4 
0.4 
0.0 
  Card 11 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OMG_P 
PHI_P 
PSI_P 
CR_P 
OMG_B 
PHI_B 
PSI_B 
CR_B 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Defaults 
0.32 
0.4 
0.4 
0.0 
0.29 
0.4 
0.4 
0.0 
Heat Card 1.  Additional Card for HEAT ≠ 0. 
  Card 12 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
AUST 
FERR 
PEAR 
BAIN 
MART 
GRK 
GRQR 
TAU1 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
2.08E+8
Heat Card 2.  Additional Card for HEAT ≠ 0. 
  Card 13 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
GRA 
GRB 
EXPA 
EXPB 
GRCC 
GRCM 
HEATN 
TAU2 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
3.11 
7520. 
1.0 
1.0 
none 
none 
1.0 
4.806
Extra Card 1.  Additional Card for IEXTRA  =  1. 
  Card 14 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FUNCA 
FUNCB 
FUNCM 
TCVUP 
TCVLO 
CVCRIT 
TCVSL 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Extra Card 2.  Additional Card for IEXTRA  =  2. 
  Card 15 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EPSP 
EXPON 
Type 
F 
F 
Default 
0.0 
0.0 
VARIABLE 
DESCRIPTION 
BASELINE VALUE 
MID 
RO 
Material  ID,  a  unique  number  has  to  be 
chosen. 
Material  density  at  room  temperature 
(necessary  for  calculating  transformation 
induced strains) 
7830 Kg/m3
E 
Youngs’ modulus: 
100.e+09 Pa [1]
GT.0.0: constant value is used 
LT.0.0:  LCID  or  TABID.    Temperature 
dependent  Young’s  modulus 
given  by  load  curve  or  table 
ID = -E.  When using a table to 
describe  the  Young’s  modulus 
see  Remark  10  for  more  infor-
mation.
VARIABLE 
DESCRIPTION 
BASELINE VALUE 
PR 
Poisson’s ratio: 
0.30 [1]
3600.
0 
0 
TUNIT 
TRIP 
PHASE 
GT.0.0: constant value is used 
LT.0.0:  LCID  or  TABID.    Temperature 
dependent  Poisson’s  ratio  giv-
en by load curve or table ID = -
PR.    The  table  input  is  de-
scribed in Remark 10. 
Number  of  time  units  per  hour.    Default 
is  seconds,  that  is  3600  time  units  per 
hour. 
  It  is  used  only  for  hardness 
calculations. 
Flag  to  activate  (0)  or  deactivate  (1)  trip 
effect calculation.  
Switch to exclude middle phases from the 
simulation. 
EQ.0: all phases active (default) 
EQ.1: pearlite and bainite active 
EQ.2: bainite active 
EQ.3: ferrite and pearlite active 
EQ.4: ferrite and bainite active 
EQ.5: no active middle phases  
(only austenite → martensite) 
HEAT 
Heat  flag  as  in  MAT_244,  see  there  for 
details. 
EQ.0: Heating is not activated. 
EQ.1: Heating is activated. 
EQ.2: Automatic  switching  between 
cooling and heating. 
LT.0:  Switch  between  cooling  and 
heating  is  defined  by  a  time  de-
id 
pendent 
ABS(HEAT). 
load  curve  with
LCY1 
LCY2 
LCY3 
LCY4 
LCY5 
C_F 
C_P 
C_B 
C 
Co 
Mo 
*MAT_PHS_BMW 
DESCRIPTION 
BASELINE VALUE 
Load  curve  or  Table  ID  for  austenite 
hardening. 
if LCID 
input  yield  stress  versus  effective 
plastic strain. 
if TABID.GT.0: 
2D table.  Input temperatures as table 
values  and  hardening  curves  as 
targets  for  those  temperatures   
if TABID.LT.0: 
3D table.  Input temperatures as main 
table values and strain rates as values 
for  the  sub  tables,  and  hardening 
curves as targets for those strain rates. 
Load  curve  or  Table  ID  for  ferrite.    See 
LCY1 for description. 
Load  curve  or  Table  ID  for  pearlite.    See 
LCY1 for description. 
Load  curve  or  Table  ID  for  bainite.    See 
LCY1 for description. 
Load  curve  or  Table  ID  for  martensite.  
See LCY1 for description. 
for  ferrite 
Alloy  dependent  factor  𝐶𝑓
(controls  the  alloying  effects  beside  of 
Boron 
time-temperature-
the 
transformation start line of ferrite). 
on 
Alloy  dependent  factor  𝐶𝑝 for  pearlite 
. 
Alloy dependent factor 𝐶𝑏 for bainite . 
Carbon [weight %]
Cobolt [weight %]
Molybdenum [weight %]
[5]
0.23 [2, 4]
0.0 [2, 4]
0.0 [2, 4]
VARIABLE 
DESCRIPTION 
BASELINE VALUE 
Cr 
Ni 
Mn 
Si 
V 
W 
Cu 
P 
Al 
As 
Ti 
Β 
TABRHO 
TREF 
LAT1 
Chromium [weight %]
Nickel [weight %]
Manganese [weight %]
Silicon [weight %]
Vanadium [weight %]
Tungsten [weight %]
Copper [weight %]
Phosphorous [weight %]
Aluminium [weight %]
Arsenic [weight %]
Titanium [weight %]
Boron [weight %]
for 
definition 
and 
Table 
temperature 
densities.  
Needed  for  calculation  of  transformation 
induced strains. 
dependent 
phase 
temperature 
Reference 
thermal 
expansion  (only  necessary  for  thermal 
expansion  calculation  with  the  secant 
method). 
for 
0.21 [2, 4]
0.0 [2, 4]
1.25 [2, 4]
0.29 [2, 4]
0.0 [2, 4]
0.0
0.0
0.013
0.0
0.0
0.0
0.0
293.15
Latent  heat  for  the  decomposition  of 
austenite into ferrite, pearlite and bainite. 
GT.0.0: Constant value 
590.e+06 J/m3 [2]
LT.0.0:  Curve  ID  or  Table  ID:  See 
infor-
for  more 
remark  11 
mation.
640.e+06 J/m3 [2]
*MAT_248 
VARIABLE 
LAT5 
DESCRIPTION 
Latent  heat  for  the  decomposition  of 
austenite into martensite. 
GT.0.0: Constant value 
LT.0.0:  Curve ID: Note  that  LAT  5  is 
ignored if a Table ID is used in 
LAT1. 
TABTH 
Table  definition  for  thermal  expansion 
coefficient. 
for  more 
  See  remarks 
information how to input this table. 
QR2 
QR3 
QR4 
ALPHA 
GT.0:  A 
for 
table 
instantaneous 
thermal  expansion  (TREF  is  ig-
nored). 
LT.0:  A  table  with  thermal  expansion 
with reference to TREF. 
energy  divided  by 
Activation 
the 
universal  gas  constant  for  the  diffusion 
reaction  of  the  austenite-ferrite  reaction: 
Q2/R.  R = 8.314472 [J/mol K]. 
energy  divided  by 
the 
Activation 
universal  gas  constant  for  the  diffusion 
reaction 
austenite-pearlite 
the 
reaction: Q3/R.  R = 8.314472 [J/mol K]. 
for 
energy  divided  by 
Activation 
the 
universal  gas  constant  for  the  diffusion 
reaction for the austenite-bainite reaction: 
Q4/R.  R = 8.314472 [J/mol K]. 
for 
Material  constant 
the  martensite 
phase.    A  value  of  0.011  means  that  90% 
of  the  available  austenite  is  transformed 
into  martensite  at  210  degrees  below  the 
,  whereas  a 
value 
99.9% 
0.033  means 
transformation. 
temperature 
start 
of 
a 
10324 K [3] =
(23000 cal/mole) × 
(4.184 J/cal) / 
(8.314 J/mole/K) 
13432.  K [3]
15068.  K [3]
0.011
GRAIN 
ASTM grain size number 𝐺 for austenite, 
usually a number between 7 and 11. 
6.8
DESCRIPTION 
BASELINE VALUE 
VARIABLE 
TOFFE 
TOFPE 
TOFBA 
PLMEM2 
PLMEM3 
PLMEM4 
PLMEM5 
STRC 
Number  of  degrees  that  the  ferrite  is 
bleeding  over  into  the  pearlite  reaction: 
𝑇off,𝑓 . 
Number  of  degrees  that  the  pearlite  is 
bleeding  over  into  the  bainite  reaction: 
𝑇off,𝑝. 
Number  of  degrees  that  the  bainite  is 
the  martensite 
into 
bleeding  over 
reaction: 𝑇off,𝑏. 
Memory  coefficient  for  the  plastic  strain 
that is carried over from the austenite.  A 
value  of  1  means  that  all  plastic  strains 
from austenite is transferred to the ferrite 
phase  and  a  value  of  0  means  that 
nothing is transferred. 
Same  as  PLMEM2  but  between  austenite 
and pearlite. 
Same  as  PLMEM2  but  between  austenite 
and bainite. 
Same  as  PLMEM3  but  between  austenite 
and martensite. 
Cowper 
parameter 𝐶. 
and  Symonds 
strain 
rate 
STRC.LT.0.0:  load curve id = -STRC  
STRC.GT.0.0:  constant value 
STRC.EQ.0.0:  strain rate NOT active 
STRP 
Cowper 
parameter P. 
and  Symonds 
strain 
rate 
STRP.LT.0.0:  load curve id = -STRP 
STRP.GT.0.0: constant value 
STRP.EQ.0.0: strain rate NOT active 
0.0
0.0
0.0
0.0
0.0
0.0
0.0
0.0
0.0
VARIABLE 
DESCRIPTION 
BASELINE VALUE 
FS 
Manual start temperature ferrite, 𝐹𝑆.  
GT.0.0: Same  temperature  is  used  for 
heating and cooling.  
LT.0.0:  Curve ID: Different 
start 
temperatures  for  cooling  and 
heating  given  by  load  curve 
ID = -FS.  First ordinate value is 
used  for  cooling,  last  ordinate 
value for heating. 
Manual  start  temperature  pearlite,  𝑃𝑆.  
See FS for description. 
Manual start temperature bainite, 𝐵𝑆.  See 
FS for description. 
Manual start temperature martensite, 𝑀𝑆.  
See FS for description. 
Describes  the  increase  of  martensite  start 
temperature  for  cooling  due  to  applied 
stress. 
LT.0: Load Curve ID describes MSIG as 
a  function  of  triaxiality  (pressure 
/ effective stress). 
MS* = MS + MSIG × 𝜎eff
Load  Curve  ID  dependent  on  plastic 
strain  that  scales  the  activation  energy 
QR2 and QR3. 
QRn = Qn × LCEPS23(𝜀pl)/𝑅
Load  Curve  ID  dependent  on  plastic 
strain  that  scales  the  activation  energy 
QR4. 
QR4 = Q4 × LCEPS4(𝜀pl)/𝑅
PS 
BS 
MS 
MSIG 
LCEPS23 
LCEPS4
VARIABLE 
LCEPS5 
LCH4 
LCH5 
DTCRIT 
TSAMP 
ISLC 
DESCRIPTION 
BASELINE VALUE 
ID  which  describe 
the  martensite 
the 
Load  Curve 
increase 
start 
of 
temperature  for  cooling  as  a  function  of 
plastic strain. 
MS* = MS + MSIG × 𝜎eff + LCEPS5(𝜀pl) 
Load  curve  ID  of  Vickers  hardness  vs.  
temperature 
hardness 
calculation. 
bainite 
for 
Load  curve  ID  of  Vickers  hardness  vs.  
temperature 
for  martensite  hardness 
calculation. 
Critical  cooling  rate  to  detect  holding 
phase. 
Sampling  interval  for  temperature  rate 
monitoring to detect the holding phase 
for 
Flag 
parameters on Cards 10 and 11. 
definition 
of 
evolution 
EQ.0.0:   All 16 parameters on Cards 10 
and 11 are constant values. 
EQ.1.0:   PHI_F,  CR_F,  PHI_P,  CR_P, 
PHI_B,  and  CR_B  are  load 
curves  defining  values  as 
functions  of  cooling  rate.    The 
remaining  10  paramters  on 
Cards  10  and  11  are  constant 
values.  
EQ.2.0:   All 16 parameters on Cards 10 
and  11  are  load  curves  defin-
ing values as functions of cool-
ing rate. 
IEXTRA 
Flag to read extra cards 
ALPH_M 
Martensite evolution parameter 𝛼𝑚 
N_M 
PHI_M 
Martensite evolution parameter 𝑛𝑚 
Martensite evolution parameter 𝜑𝑚 
0.0428 
0.191 
0.382
PSI_M 
OMG_F 
PHI_F 
PSI_F 
CR_F 
OMG_P 
PHI_P 
PSI_P 
CR_P 
OMG_B 
PHI_B 
PSI_B 
CR_B 
*MAT_PHS_BMW 
DESCRIPTION 
BASELINE VALUE 
Martensite  evolution  exponent  𝜓𝑚, 
𝜓𝑚 < 0 then 𝜓𝑚 = ∣𝜓𝑚∣(2 − 𝜍𝑎) 
if 
Ferrite  grain  size  factor  𝜔𝑓   (mainly 
controls  the  alloying  effect  of  Boron  on 
the time-temperature-transformation start 
line of ferrite) 
Ferrite  evolution  parameter  𝜑𝑓   (controls 
the incubation time till 1vol% of ferrite is 
built) 
Ferrite  evolution  parameter  𝜓𝑓   (controls 
the  time  till  99vol%  of  ferrite  is  built 
without effect on the incubation time) 
evolution 
parameter 
Ferrite 
𝐶𝑟,𝑓  
(retardation  coefficient  to  influence  the 
kinetics of phase transformation of ferrite, 
should  be  determined  at  slow  cooling 
in 
conditions,  can  also  be  defined 
dependency to the cooling rate) 
Pearlite  grain  size  factor  𝜔𝑝   
Pearlite  evolution  parameter  𝜑𝑝 
PHI_F for description) 
 
Pearlite  evolution  parameter  𝐶𝑟,𝑝   
Bainite  grain  size  factor  𝜔𝑏   
Bainite evolution parameter 𝜑𝑏  
Bainite evolution parameter 𝜓𝑏  
Bainite  evolution  parameter  𝐶𝑟,𝑏
CR_F for description) 
(see 
2.421 
0.41 
0.4 
0.4 
0.0 
0.32 
0.4 
0.4 
0.0 
0.32 
0.4 
0.4 
0.0
DESCRIPTION 
BASELINE VALUE 
VARIABLE 
AUST 
FERR 
PEAR 
BAIN 
MART 
GRK 
GRQR 
TAU1 
GRA 
GRB 
EXPA 
EXPB 
GRCC 
GRCM 
If  a  heating  process  is  initiated  at  t = 0 
this  parameters  sets  the  initial  amount  of 
austenite  in  the  blank.    If  heating  is 
activated at t > 0 during a simulation this 
value is ignored.  Note that, 
AUST + FERR + PEAR
+ BAIN + MART 
= 1.0
See AUST for description
See AUST for description
See AUST for description
See AUST for description
Growth parameter k (μm2/sec)
Grain  growth  activation  energy  (J/mol) 
divided  by  the  universal  gas  constant.  
Q/R where R = 8.314472 (J/mol K) 
Empirical  grain  growth  parameter  𝑐1
describing the function τ(T) 
Grain growth parameter A
Grain  growth  parameter  B.    A  table  of 
recommended values of GRA and GRB is 
included in Remark 7 of *MAT_244. 
Grain growth parameter 𝑎
Grain growth parameter 𝑏
Grain  growth  parameter  with 
the 
concentration  of  non  metals  in  the  blank, 
weight% of C or N  
Grain  growth  parameter  with 
the 
concentration  of  metals  in  the  blank, 
lowest weight% of Cr, V, Nb, Ti, Al. 
0.0
0.0
0.0
0.0
0.0
1.0E+11[9]
3.0E+4[9]
2.08E+8 [9]
 [9]
 [9]
1.0 [9]
1.0 [9]
 [9]
 [9]
1.0[9]
HEATN 
Grain  growth  parameter  𝑛 for 
austenite formation 
the
BASELINE VALUE 
Empirical  grain  growth  parameter  𝑐2
describing the function τ(T) 
4.806[9]
ID  of  a 
saturation 
approach) 
*DEFINE_FUNCTION 
stress  A 
for 
(Hockett-Sherby 
ID  of  a  *DEFINE_FUNCTION  for    initial 
yield stress B (Hockett-Sherby approach) 
ID  of  a 
saturation 
approach) 
*DEFINE_FUNCTION 
rate  M 
for 
(Hockett-Sherby 
Upper  temperature  for  determination  of 
average cooling velocity 
Lower  temperature  for  determination  of 
average cooling velocity 
Critical  cooling  velocity.    If  the  average 
cooling  velocity 
is  smaller  or  equal 
CVCRIT,  the  cooling  rate  at  TCVSL  is 
used. 
Temperature for determination of cooling 
velocity for small cooling velocities. 
Plastic strain in Hockett-Sherby approach
Exponent in Hockett-Sherby approach
*MAT_248 
VARIABLE 
TAU2 
FUNCA 
FUNCB 
FUNCM 
TCVUP 
TCVLO 
CVCRIT 
TCVSL 
EPSP 
EXPON 
Remarks: 
1.  Start  Temperatures.    Start  temperatures  for  ferrite,  pearlite,  bainite,  and 
martensite can be defined manually via FS, PS, BS, and MS.  Or they are initially 
defined using the following composition equations: 
𝐹𝑆 = 273.15 + 912 − 203 × √C − 15.2 × Ni + 44.7 × Si + 104 × V + 31.5 × Mo
+ 13.1 × W − 30 × Mn − 11 × Cr − 20 × Cu + 700 × P + 400 × Al
+ 120 × As + 400 
𝑃𝑆 = 273.15 + 723 − 10.7 × Mn − 16.9 × Ni + 29 × Si + 16.9 × Cr + 290 × As
+ 6.4 × W 
𝐵𝑆 = 273.15 + 637 − 58 × C − 35 × Mn − 15 × Ni − 34 × Cr − 41 × Mo
𝑀𝑆 = 273.15 + 539 − 423 × C − 30.4 × Mn − 17.7 × Ni − 12.1 × Cr − 7.5 × Mo
+ 10 × Co − 7.5 × Si 
2.  Martensite Phase Evolution.  Martensite phase evolution according to Lee et 
al.  [2008, 2010] if PSI_M > 0: 
d𝜉𝑚
d𝑇
= α𝑚(𝑀𝑆 − 𝑇)𝑛𝜉𝑚
𝜑𝑚(1 − 𝜉𝑚)𝜓𝑚 
Martensite phase evolution according to Lee et al.  [2008, 2010] with extension 
by Hippchen et al.  [2013] if PSI_M < 0:  
d𝜉𝑚
d𝑇
= α𝑚(𝑀𝑆 − 𝑇)𝑛𝜉𝑚
𝜑𝑚(1 − 𝜉𝑚)𝜓𝑚(2−𝜁𝑎) 
3.  Phase Change Kinetics for Ferrite, Pearlite and Bainite. 
d𝜉𝑓
d𝑡
= 2𝜔𝑓 𝐺
exp (−
𝑄𝑓
𝑅𝑇
)
𝐶𝑓
(𝐹𝑆 − 𝑇)3
𝜓𝑓 𝜉𝑓
𝜉 𝜑𝑓 (1−𝜉𝑓 )(1 − 𝜉𝑓 )
2)
exp(𝐶𝑟,𝑓 𝜉𝑓
for   𝐹𝑆 ≥ 𝑇 ≥ (𝑃𝑆 − 𝑇off,𝑓 ) 
d𝜉𝑝
d𝑡
= 2𝜔𝑝𝐺
exp (−
𝑄𝑝
𝑅𝑇
)
𝐶𝑝
(𝑃𝑆 − 𝑇)3
𝜓𝑝𝜉𝑝
𝜉 𝜑𝑝(1−𝜉𝑝)(1 − 𝜉𝑝)
2)
exp(𝐶𝑟,𝑝𝜉𝑝
for   𝑃𝑆 ≥ 𝑇 ≥ (𝐵𝑆 − 𝑇off,𝑝) 
d𝜉𝑏
d𝑡
= 2𝜔𝑏𝐺
exp (−
𝑄𝑏
𝑅𝑇
)
𝐶𝑏
(𝐵𝑆 − 𝑇)2 𝜉 𝜑𝑏(1−𝜉𝑏)(1 − 𝜉𝑏)𝜓𝑏𝜉𝑏
exp(𝐶𝑟,𝑏𝜉𝑏
2)
for   𝑀𝑆 ≥ 𝑇 ≥ (𝑀𝑆 − 𝑇off,𝑏)
4.  History  Variables.    History  variables  of  this  material  model  are  listed  in  the 
following table.  To be able to post-process that data, parameters NEIPS (shells) 
or NEIPH (solids) have to be defined on *DATABASE_EXTENT_BINARY. 
History 
Variable 
Description 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
11 
12 
13 
17 
19 
25 
26 
Amount austenite 
Amount ferrite 
Amount pearlite 
Amount bainite 
Amount martensite 
Vickers hardness 
Yield stress 
ASTM grain size number 
Young’s modulus 
Saturation stress A (H-S approach) 
Initial yield stress B (H-S approach) 
Saturation rate M (H-S approach) 
Yield stress of H-S approach 
𝜎𝑦 = 𝐴 − (𝐴 − 𝐵) ∙ 𝑒−𝑀∙𝐸𝑃𝑆𝑃𝐸𝑋𝑃𝑂𝑁
Temperature rate 
Current temperature 
Plastic strain rate 
Effective thermal expansion coefficient 
5.  Choosing/Excluding Phases.  To exclude a phase from the simulation, set the 
PHASE parameter accordingly. 
6.  Strain  Rate  Effects.    Note  that  both  strain  rate  parameters  (STRC  and  STRP) 
must be set to include the effect.  It is possible to use a temperature dependent 
load  curve  for  both  parameters  simultaneously  or  for  one  parameter  keeping 
the other constant. 
7.  Time Units.  TUNIT is time units per hour and is only used for calculating the 
Vicker Hardness, as default it is assumed that the time unit is seconds.  If other
time  unit  is  used,  for  example  milliseconds,  then  TUNIT  must  be  changed  to 
TUNIT = 3.6 × 106 
8.  Thermal  Speedup  Factor.    The  thermal  speedup  factor  TSF  of  *CONTROL_-
THERMAL_SOLVER  is  used  to  scale  reaction  kinetics  and  hardness  calcula-
tions  in  this  material  model.    On  the  other  hand,  strain  rate  dependent 
properties  are not scaled by TSF. 
9.  Re-austenization  and  Grant  Growth  with  HEAT  Option.    When  HEAT  is 
activated the re-austenitization and grain growth algorithms are also activated.  
See MAT_244 for details. 
10.  Phase  Indexed  Tables.    When  using  a  Table  ID  for  describing  the  Young’s 
modulus  as  dependent  on  the  temperature  Use  *DEFINE_TABLE_2D  and  set 
the abscissa value equal to 1 for the austenite YM-curve, equal to 2 for the fer-
rite  YM-curve,  equal  to  3  for  the  pearlite  YM  curve,  equal  to  4  for  the  bainite 
YM-curve and finally equal to 5 for the martensite YM-curve.  When using the 
PHASE option only the curves for the included phases are required, but all five 
phases may be included.  The total YM is calculated by a linear mixture law:  
YM = YM1 × PHASE1 + ⋯ + YM5 × PHASE5 
For example: 
*DEFINE_TABLE_2D 
$ The number before curve id:s define which phase the curve 
$ will be applied to.  1 = Austenite, 2 = Ferrite, 3 = Pearlite, 
$ 4 = Bainite and 5 = Martensite.  
      1000       0.0       0.0 
                 1.0                 100 
                 2.0                 200 
                 3.0                 300 
                 4.0                 400 
                 5.0                 500 
$ 
$ Define curves 100 - 500 
*DEFINE_CURVE 
$ Austenite Temp (K) - YM-Curve (MPa) 
       100         0       1.0       1.0 
              1300.0              50.E+3 
               223.0             210.E+3 
11.  Phase-indexed Latent Heat Table.  A Table ID may be specified for the Latent 
heat  (LAT1)  to  describe  each  phase  change  individually.    Use  *DEFINE_TA-
BLE_2D and set the abscissa values to the corresponding phase transition num-
ber.  That is, 2 for the Austenite – Ferrite, 3 for the Austenite – Pearlite,’4’ for the 
Austenite – Bainite and 5 for the Austenite – Martensite.  See Remark 7 for an 
example  of  a  correct  table  definition.    If  a  curve  is  missing,  the  corresponding 
latent heat for that transition will be set to zero.  Also, when a table is used the 
LAT2 is ignored.  If HEAT.GT.0 you also have the option to include latent heat
for the transition back to Austenite.  This latent heat curve is marked as 1 in the 
table definition of LAT1. 
12.  Phase-indexed Thermal Expansion Table.  Tables are supported for defining 
different thermal expansion properties for each phase.  The input is identical to 
the above table definitions.  The Table must have the abscissa values between 1 
and 5 where the number correspond to phase 1 to 5.  To exclude one phase from 
influencing the thermal expansion you simply input a curve that is zero for that 
phase  or  even  easier,  exclude  that  phase  number  in  the  table  definition.    For 
example to exclude the bainite phase you only define the table with curves for 
the indices 1, 2, 3 and 5. 
13.  Phase-indexed Transformation Induced Strain Properties.  Transformation 
induced  strains  can  be  define  with  a  table  TABRHO,  where  densities  are  de-
fined as functions of phase (table abscissas) and temperature (load curves).
*MAT_REINFORCED_THERMOPLASTIC 
This  is  material  type  249.    This  material  model  describes  a  reinforced  thermoplastic 
composite  material.    The  reinforcement  is  defined  as  an  anisotropic  hyper-elastic 
material  with  up  to  three  distinguished  fiber  directions.    It  can  be  used  to  model 
unidirectional layers as well as woven and non-crimped fabrics.  The matrix is modeled 
with a simple thermal elasto-plastic material formulation.  For a composite an additive 
composition of fiber and matrix stresses is used.   
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
Variable 
NFIB 
AOPT 
Type 
I 
F 
  Card 3 
Variable 
1 
V1 
Type 
F 
  Card 4 
1 
2 
V2 
F 
2 
3 
4 
5 
6 
7 
8 
EM 
LCEM 
PRM 
LCPRM 
LCSIGY 
BETA 
F 
I 
F 
I 
I 
F 
3 
XP 
F 
3 
V3 
F 
3 
4 
YP 
F 
4 
D1 
F 
4 
5 
ZP 
F 
5 
D2 
F 
5 
6 
A1 
F 
6 
7 
A2 
F 
7 
8 
A3 
F 
8 
D3 
MANGL 
THICK 
F 
6 
F 
7 
F 
8 
Variable 
IDF1 
ALPH1 
EF1 
LCEF1 
G23_1 
G31_1 
Type 
I 
F 
F 
I 
F
Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
G12 
LCG12 
ALOC12  GLOC12  METH12 
Type 
F 
  Card 6 
1 
I 
2 
F 
3 
F 
4 
I 
5 
6 
7 
8 
Variable 
IDF2 
ALPH2 
EF2 
LCEF2 
G23_2 
G31_2 
Type 
I 
  Card 7 
1 
F 
2 
F 
3 
I 
4 
F 
5 
F 
6 
7 
8 
Variable 
G23 
LCG23 
ALOC23  GLOC23  METH23 
Type 
F 
  Card 8 
1 
I 
2 
F 
3 
F 
4 
I 
5 
6 
7 
8 
Variable 
IDF3 
ALPH3 
EF3 
LCEF3 
G23_3 
G31_3 
Type 
I 
F 
F 
I 
F 
F 
The following card is optional 
  Card 9 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
POSTV 
Type 
F 
  VARIABLE   
MID 
2-1256 (MAT_248) 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
VARIABLE   
DESCRIPTION
RO 
EM 
LCEM 
PR 
LCPR 
Density. 
Young’s modulus of matrix material. 
Curve  ID  for  Young’s  modulus  of  matrix  material  versus
temperature.  With this option active, EM is ignored.  
Poisson’s ratio for matrix material 
Curve 
temperature.  With this option active, PR is ignored. 
for  Poisson’s  ratio  of  matrix  material  versus
ID 
LCSIGY 
Load curve or table ID for strain hardening of the matrix. 
IF LCSIGY refers to a curve 
Input yield stress versus effective plastic strain. 
IF LCSIGY refers to a table: 
Input temperatures as table values and hardening curves 
as targets for those temperatures  
BETA 
Parameter  for  mixed  hardening.    Set  𝛽 = 0  for  pure  kinematic 
hardening and 𝛽 = 1 for pure isotropic hardening. 
NFIB 
Number of fiber families to be considered.
AOPT 
*MAT_REINFORCED_THERMOPLASTIC 
DESCRIPTION
Material axes option : 
EQ.0.0:  locally  orthotropic  with  material  axes  determined  by 
element  nodes,  as  with  *DEFINE_COORDI-NATE_-
NODES, and then rotated about the shell element nor-
mal by the angle MANGL. 
EQ.2.0:  globally  orthotropic  with  material  axes  determined  by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0:  locally  orthotropic  material  axes  determined  by
rotatingthe material axes about the element normal by
an  angle,  MANGL,  from  a  line  in  the  plane of  the  ele-
ment defined by the cross product of the vector v with
the element normal 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR). 
XP, YP, ZP 
Coordinates of point 𝐩 for AOPT = 1. 
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3. 
D1, D2, D3 
Components of vector 𝐝 for AOPT = 2. 
MANGL 
THICK 
Material angle in degrees for AOPT = 0 and 3, may be overwritten 
on the element card, see *ELEMENT_SHELL_BETA. 
Balance  thickness  changes  of  the  material  due  to  the  matrix 
description by scaling fiber stresses 
EQ.0:  No scaling  
EQ.1:  Scaling 
IDFi 
ID for i-th fiber family for post-processing 
ALPHi 
Orientation angle 𝛼𝑖 for i-th fiber with respect to overall material 
direction 
EFi 
Young’s modulus for i-th fiber family
VARIABLE   
DESCRIPTION
LCEFi 
G23_i 
G31_i 
Gij 
LCGij 
Curve ID for stress versus fiber elongation of i-th fiber.  With this 
option active, EFi is ignored. 
Transversal shear modulus orthogonal to direction of fiber i 
Transversal shear modulus in direction of fiber i 
Linear shear modulus for shearing between fiber i and j 
Curve ID for shear stress versus shearing between of i-th and j-th 
fiber.    With  this  option  active,  Gij  is  ignored.    For  details  see 
parameter METHij. 
ALOCij 
Locking angle (in radians) for shear between fiber families i and j
GLOCij 
Linear shear modulus for shear angles larger than ALOCij 
METHij 
Option for shear between fiber i and j : 
EQ.0:  Elastic  shear  response,  curve  LCGij  defines  shear 
stress vs. scalar product of fibers directions.  
EQ.1 
Elasto-plastic shear response, curve LCGij defines yield 
shear stress vs.  normalized scalar product of fiber di-
rections. 
EQ.2:  Elastic  shear  response,  curve  LCGij  defines  shear 
stress vs.  shear angle between fibers given in rad. 
EQ.3:   Elasto-plastic shear response, curve LCGij defines yield 
shear  stress  vs.    normalized  shear  angle  between  fi-
bers.  
EQ.4:  Elastic  shear  response,  curve  LCGij  defines  shear 
stress  vs.    shear  angle  between  fibers  given  in  rad.
This  option  is  a  special  implementation  for  non-
crimped fabrics, where one of the fiber families corre-
sponds to a stitching. 
EQ.5:   Elasto-plastic shear response, curve LCGij defines yield 
shear  stress  vs.    normalized  shear  angle  between  fi-
bers.  This option is a special implementation for non-
crimped fabrics, where one of the fiber families corre-
sponds to a stitching. 
EQ.10:   Elastic  shear  response,  curve  LCGij  defines  shear 
stress  vs.    shear  angle  between  fibers  given  in  rad.
This  option  is  tailored  for  woven  fabrics  and  guaran-
tees a pure shear stress response.
*MAT_REINFORCED_THERMOPLASTIC 
DESCRIPTION
EQ.11:  Elasto-plastic  shear  response,  curve  LCGij  defines 
yield  shear  stress  vs.    normalized  shear  angle.    This
option  is  tailored  for  woven  fabrics  and  guarantees  a
pure shear stress response 
POSTV 
Defines additional history variables that might be useful for post-
processing.  See remarks below for details. 
Stress calculation: 
This  material  features  an  additive  split  of  matrix  and  reinforcement  contributions,  i.e.  
the  combined  stress  response  𝝈  equals  the  sum 𝝈𝑚 + 𝝈𝑓 .    The  matrix  mechanics  is 
described by an elasto-plastic material formulation with a von-Mises yield criterion.  
The  contribution  of  the  reinforcement  is  formulated  as  a  hyperelastic  material.    Based 
0  is 
on  the  orientation  angel  𝛼𝑖  of  the  i-th  fiber  family  an  initial  fiber  direction  𝐦𝑖
computed.    By  using  the  deformation  gradient  𝐅  the  current  fiber  configuration  is 
0  containing  all  necessary  information  on  fiber  strain  and 
defined  as  𝐦i = 𝐅 𝐦𝑖
reorientation.  
Following standard textbook mechanics for anisotropic and hyperelastic materials, the 
elastic stresses within the fibers due to tension or compression are given as  
𝑓 = ∑
𝑖=1
where the function 𝑓𝑖 of the fiber stretch 𝜆𝑖 corresponds to the load curve LCEFi.  
, 
𝑓𝑖(𝜆𝑖)(𝐦i ⊗ 𝐦i)
𝝈𝑇
The  shear  behavior  of  the  reinforcement  can  be  controlled  by  METHij.  For  values  less 
than 10, the behavior is again standard textbook mechanics: 
𝝈𝑆
𝑓 = ∑
𝑖=1
𝑔𝑖,𝑖+1(𝜅𝑖,𝑖+1)(𝐦i ⊗ 𝐦i+1)
Where  𝜅𝑖,𝑖+1  represents  the  employed  shear  measure  (scalar  product  or  shear  angle  in 
rad).    In  general,  the  dyadic  product  𝐦i ⊗ 𝐦i+1  does  not  define  a  shear  stress  tensor.  
This  might  result  in  unphysical  shear  behavior  in  case  of  woven  fabrics.    Therefore, 
𝑓  is always 
METHij = 10 or 11 have been devised such that a pure shear stress tensor 𝝈𝑆
obtained.  
For even values of METHij, an elastic  shear response is assumed.   If defined, the load 
curve  LCGij  corresponds  to  function  𝑔𝑖,𝑗.    In  this  case  the  values  of  Gij,  ALOCij  and 
GLOCij are ignored.
For  odd  values  of  METHij  on  the  other  hand,  an  elasto-plastic  shear  behavior  is 
assumed  and  the  load  curve  LCGij  defines  the  yield  stress  value  as  function  of  a 
normalized  shear  parameter.    This  implies  that  the  load  curve  has  to  be  defined  for 
abscissa  values  between  0.0  and  1.0.    A  first  elastic  regime,  which  is  controlled  by  the 
linear  shear  stiffness  Gij,  is  assumed  until  the  yield  stress  given  in  the  load  curve  for 
normalized  shear  value  0.0  is  reached.    A  second  linear  elastic  regime  is  defined  for 
shear  angles  (𝜉𝑖𝑗)/  fiber  angles  (𝜂𝑖𝑗)  larger  than  the  locking  angle  ALOCij.    The 
corresponding stiffness in that regime is GLOCij. At the transition point to the second 
elastic  regime,  the  shear  stress  corresponds  to  the  load  curve  value  for  a  normalized 
shear of 1.0. 
History data: 
This  material  formulation  outputs  additional  data  for  post-processing  to  the  set  of 
history variables if requested by the user.  The parameter POSTV defines the data to be 
written.  Its value is calculated as 
POSTV = a1 + 2 𝑎2 + 4 𝑎3 + 8 𝑎4 + 16 𝑎5 + 32 𝑎6. 
Each  flag   𝑎𝑖  is  a  binary  (can  be  either  1  or  0)  and  corresponds  to  one  particular  post-
processing variable according to the following table. 
Flag 
Description 
Variables 
# hist 
𝑎1 
𝑎2 
𝑎3 
𝑎4 
𝑎5 
𝑎6 
Fiber angle 
Fiber ID 
Fiber stretch 
Fiber direction 
𝜂12, 𝜂23 
IDF1, IDF2, IDF3 
𝜆1, 𝜆2, 𝜆3 
𝐦1, 𝐦2, 𝐦3 
Individual fiber stresses 
𝑓1(𝜆1), 𝑓2(𝜆2), 𝑓3(𝜆3) 
Fiber stress tensor 
,  𝜎22
,  𝜎33
,  𝜎12
,  𝜎23
, 
𝜎11
𝜎31
2 
3 
3 
9 
3 
6 
The above table also shows the order of output as well as the number of extra history 
variables associated with the particular flag.  In total NXH extra variables are required 
depending on the choice of parameter POSTV.  For example, the maximum number of 
additional variables is NXH = 26 for POSTV = 63. 
The post-processing data are written prior to most of the algorithmic history variables.  
A list of potentially helpful history variables are given in the following table.
Position 
Description 
3  Number of Fibers 
4  NXH 
5→NXH+4  Extra post-processing output 
NXH+5, NXH+6 
Shear angles 𝜉12and 𝜉23 
NXH+7 → NXH+12  Matrix stress tensor  
NXH+13 → NXH+21  Deformation gradient
This  is  material  type  249.    It  describes  a  material  with  unidirectional  fiber  reinforce-
ments  and  considers  up  to  three  distinguished  fiber  directions.    Each  fiber  family  is 
described  by  a  spatially  transversely  isotropic  neo-Hookean  constitutive  law.    The 
implementation is based on an adapted version of the material described by Bonet and 
Burton  (1998).  The  material  is  only  available  for  thin  shell  elements  and  in  explicit 
simulations. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
Variable 
NFIB 
AOPT 
Type 
I 
F 
  Card 3 
Variable 
1 
V1 
Type 
F 
  Card 4 
1 
2 
V2 
F 
2 
3 
EM 
4 
PRM 
F 
F 
3 
XP 
F 
3 
V3 
F 
3 
4 
YP 
F 
4 
D1 
F 
4 
Variable 
IDF1 
ALPH1 
EF1 
KAP1 
Type 
I 
F 
F 
F 
5 
G 
F 
5 
ZP 
F 
5 
D2 
F 
5 
6 
7 
8 
EZDEF 
F 
6 
A1 
F 
6 
7 
A2 
F 
7 
D3 
MANGL 
F 
6 
F 
7 
8 
A3 
F 
8
*MAT_249_UDFIBER  *MAT_REINFORCED_THERMOPLASTIC_UDFIBER 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IDF2 
ALPH2 
EF2 
KAP2 
Type 
I 
F 
F 
F 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IDF3 
ALPH3 
EF3 
KAP3 
Type 
I 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
EM 
PR 
G 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Density. 
Isotropic young’s modulus 𝐸iso. 
Poisson’s ratio 𝑣. 
Linear shear modulus 𝐺fib. 
EZDEF 
Algorithmic  parameter.    If  set  to  1,  last  row  of  deformation
gradient is not updated during the calculation. 
NFIB 
Number of fiber families to be considered.
*MAT_REINFORCED_THERMOPLASTIC_UDFIBER  *MAT_249_UDFIBER 
  VARIABLE   
AOPT 
DESCRIPTION
Material  axes  option  : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element 
with
nodes, 
*DEFINE_COORDINATE_NODES,  and  then  rotated
about the shell element normal by the angle MANGL. 
as 
EQ.2.0:  globally  orthotropic  with  material  axes  determined  by
with 
below, 
vectors 
defined 
*DEFINE_COORDINATE_VECTOR. 
as 
EQ.3.0:: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, MANGL, from a line in the  plane  of the ele-
ment defined by the cross product of the vector v with 
the element normal 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES,
*DEFINE_COORDINATE_SYSTEM 
or
*DEFINE_COORDINATE_VECTOR). 
XP, YP, ZP 
Coordinates of point p for AOPT = 1. 
A1, A2, A3 
Components of vector a for AOPT = 2. 
V1, V2, V3 
Components of vector v for AOPT = 3. 
D1, D2, D3 
Components of vector d for AOPT = 2. 
MANGL 
Material angle in degrees for AOPT = 0 and 3, may be overwritten 
on the element card, see *ELEMENT_SHELL_BETA. 
IDFi 
ID for i-th fiber family for post-processing. 
ALPHi 
EFi 
KAPi 
Orientation angle 𝛼𝑖 for i-th fiber with respect to overall material 
direction 
Young’s modulus 𝐸𝑖 for i-th fiber family. 
Fiber volume ratio 𝜅𝑖 of i-th fiber family.
*MAT_249_UDFIBER  *MAT_REINFORCED_THERMOPLASTIC_UDFIBER 
Stress calculation: 
In this model up to three distinguished fiber families are considered.  It is assumed that 
there is no interaction between the families and, thus, that the resulting stress tensor is 
given  by  the  sum  of  the  single  fiber  responses,  each  to  be  calculated  as  the  sum  of  an 
iso 
isotropic  and  a  spatially  transversely  isotropic  neo-Hookean  stress  contribution,  𝝈𝑖
tr , respectively.  The implementation is  based on the work of Bonet and Burton 
and 𝝈𝑖
(1998), adapted by BMW for simulation of unidirectional fabrics, see references below.  
In order to determine the isotropic stress tensor 𝝈𝑖
an isotropic bulk modulus 𝜆𝑖 have to be defined from the input values as:  
𝑖𝑠𝑜, an isotropic shear modulus 𝜇 and 
𝜇 =
𝐸iso
2(1 + 𝜈)
 and 𝜆𝑖 =
𝐸iso(𝜈 + 𝑛𝑖𝜈2)
. 
2(1 + 𝜈)
Here, the variable 𝑛𝑖 denotes the ratio between stiffness orthogonally to the fibers and in 
fiber direction, i.e. 𝑛𝑖 = 𝐸iso/𝐸𝑖. Using the left Cauchy-Green tensor 𝒃 the isotropic neo-
Hookean model reads: 
iso =
𝝈𝑖
(𝒃 − 𝑰) + 𝜆𝑖(𝐽 − 1)𝑰. 
0 is 
Based on the orientation angel 𝛼𝑖 of the i-th fiber family an initial fiber direction 𝐦𝑖
computed.  The deformation gradient 𝐅 is used to define the current fiber configuration 
0.    This  vector  contains  all  necessary  information  on  fiber  elongation  and 
as  𝐦i = 𝐅 𝐦𝑖
reorientation.  
The spatially transversely isotropic neo-Hookean formulation is given by:  
𝐽𝝈𝑖
tr = 2𝛽𝑖(𝐼4 − 1)𝑰 + 2(𝛼 + 2𝛽𝑖ln𝐽 + 2𝛾𝑖(𝐼4 − 1))𝐦i ⊗ 𝐦i − 𝛼(𝒃𝐦i ⊗ 𝐦i + 𝐦i ⊗ 𝒃𝐦i) 
with material parameters 
 𝛼 = 𝜇 − 𝐺fib,
𝛽𝑖 =
𝐸iso𝜈2(1 − 𝑛𝑖)
4𝑚𝑖(1 + 𝜈)
,
𝑚𝑖 = 1 − 𝜈 − 2𝑛𝑖𝜈2, 
𝛾𝑖 =
𝐸𝑖 𝜅𝑖(1 − 𝜈)
8𝑚
−
𝜆𝑖 + 2𝜇 
+
− 𝛽𝑖. 
The  parameter  EZDEF  activates  a  modification  of  the  model.    Instead  of  the  standard 
deformation  gradient  𝐅,  a  modified  tensor  𝐅̃  is  employed  to  calculate  current  fiber 
directions 𝐦i and left Cauchy-Green tensor 𝒃.  In tensor 𝐅̃ only the first two rows of the 
deformation  gradient  are  updated  based  on  the  deformation  of  the  element.    This
*MAT_REINFORCED_THERMOPLASTIC_UDFIBER  *MAT_249_UDFIBER 
simplification  can  in  some  cases  increase  the  stability  of  the  model  especially  if  the 
structure undergoes large deformations. 
References: 
-Bonet, J., and A.  J.  Burton.  "A simple orthotropic, transversely isotropic hyperelas-
tic  constitutive  equation  for  large  strain  computations."  Computer  methods  in 
applied mechanics and engineering 162.1 (1998): 151-164. 
-Senner, T., et al.  "A modular modeling approach for describing the in-plane 
forming behavior of unidirectional non-crimp-fabrics." Production Engineering 8.5 
(2014): 635-643. 
-Senner,  T.,  et  al.    "Bending  of  unidirectional  non-crimp-fabrics:  experimental 
characterization, constitutive modeling and application in finite element simula-
tion." Production Engineering 9.1 (2015): 1-10. 
 History data: 
Position 
Description 
3 
4 
5 
ID of 1st fiber 
ID of 2nd fiber 
ID of 3rd fiber 
6 → 8  Current direction of 1st fiber 
9 → 11  Current direction of 2nd fiber 
12 → 14  Current direction of 3rd fiber 
15  Number of fibers 
16  Projected orthogonal fiber strain (1st fiber) 
17  Projected parallel fiber strain (1st fiber) 
18 
Shear angle (1st fiber) in rad 
19  Euler-Almansi strain (1st fiber) 
20  Porosity (1st fiber) 
21 
Fiber volume ratio (1st fiber) 
22  Projected orthogonal fiber strain (2nd fiber) 
23  Projected parallel fiber strain (2nd fiber) 
24 
Shear angle (2nd fiber) in rad 
25  Euler-Almansi strain (2nd fiber)
*MAT_249_UDFIBER  *MAT_REINFORCED_THERMOPLASTIC_UDFIBER 
26  Porosity (2nd fiber) 
27 
Fiber volume ratio (2nd fiber) 
28  Projected orthogonal fiber strain (3rd fiber) 
29  Projected parallel fiber strain (3rd fiber) 
30 
Shear angle (3rd fiber) in rad 
31  Euler-Almansi strain (3rd fiber) 
32  Porosity (3rd fiber) 
33 
Fiber volume ratio (3rd fiber)
*MAT_251 
This is Material Type 251.  It is similar to MAT_PIECEWISE_LINEAR_PLASTICITY 
or  MAT_024  ,  except  for  the  3-D  table  option  that  uses  a 
history  variable  (e.g.    hardness,  temperature,  …)  from  a  previous  calculation  to 
evaluate the plastic behavior as a function of 1) history variable, 2) strain rate, and 3) 
plastic strain.  Only available for shell elements. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
6 
7 
8 
FAIL 
TDEL 
F 
Default 
none 
none 
none 
none 
10.E+20 
  Card 2 
1 
2 
3 
4 
Variable 
Type 
Default 
  Card 3 
1 
2 
LCSS 
F 
0 
3 
4 
5 
VP 
F 
0 
5 
6 
7 
HISVN 
PHASE 
I 
0 
6 
F 
0 
7 
F 
0 
8 
8 
Variable 
EPS1 
EPS2 
EPS3 
EPS4 
EPS5 
EPS6 
EPS7 
EPS8 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ES1 
ES2 
ES3 
ES4 
ES5 
ES6 
ES7 
ES8 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s modulus. 
Poisson’s ratio. 
FAIL 
Failure flag. 
LT.0.0:  User defined failure subroutine, matusr_24 in dyn21.F, 
is called to determine failure 
EQ.0.0: Failure is not considered.  This option is recommended
if failure is not of interest since many calculations will
be saved. 
GT.0.0:  Effective  plastic  strain  to  failure.    When  the  plastic
strain  reaches  this  value,  the  element  is  deleted  from 
the calculation. 
TDEL 
LCSS 
Minimum time step size for automatic element deletion. 
Load  curve  ID  or  Table  ID  . 
Load  curve  for  stress  vs.    plastic  strain.    2-D  table  for  stress  vs. 
plastic strain as a function of strain rates.  3-D table for stress vs. 
plastic strain as a function of strain rates as a function of history
variable values . 
VP 
Formulation for rate effects: 
EQ.0.0: Scale yield stress (default), 
EQ.1.0: Viscoplastic formulation. 
HISVN 
Location  of  history  variable  in  the  history  array  of  *INITIAL_-
STRESS_SHELL that  is used to evaluate the 3-D table LCSS.
VARIABLE   
PHASE 
EPS1 - EPS8 
DESCRIPTION
Constant  value  to  evaluate  the  3-D  table  LCSS.    Only  used  if 
HISVN = 0. 
Effective plastic strain values (optional).  At least 2 points should 
be  defined.    The  first  point  must  be  zero  corresponding  to  the
initial yield stress. 
ES1 - ES8 
Corresponding yield stress values to EPS1 - EPS8. 
Remarks: 
If  the  3-D  table  is  used  for  LCSS,  interpolation  is  used  to  find  the  corresponding 
stress  value  for  the  current  plastic  strain,  strain  rate,  and  history  variable.    In 
addition, extrapolation is used for the history variable evaluation, which means that 
some upper and lower “limit curves” have to be used, if extrapolation is not desired. 
If  material  history  is  written  to  dynain  file  using  *INTERFACE_SPRINGBACK_LS-
DYNA,  the  history  variable  of  material  251  (e.g.    hardness,  temperature,  …)  is 
written to position HISV6 of *INITIAL_STRESS_SHELL. 
It  is  recommended  to  set  HISVN = 6  and  to  put  the  history  variable  on  position 
HISV6 if *MAT_251 is used in combination with *MAT_ADD_...
*MAT_TOUGHENED_ADHESIVE_POLYMER 
This is Material Type 252, the Toughened Adhesive Polymer model (TAPO).  It is based 
on non-associated 𝐼1 - 𝐽2 plasticity constitutive equations and was specifically developed 
to  represent  the  mechanical  behaviour  of  crash  optimized  high-strength  adhesives 
under combined shear and tensile loading.  This model includes material softening due 
to  damage,  rate-dependency,  and  a  constitutive  description  for  the  mechanical 
behaviour of bonded connections under compression. 
A  detailed  description  of  this  material  can  be  found  in  Matzenmiller  and  Burbulla 
[2013].  This material model can be used with solid elements or with cohesive elements 
in combination with *MAT_ADD_COHESIVE. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
Variable 
LCSS 
TAU0 
Type 
I 
  Card 3 
1 
F 
2 
3 
E 
F 
3 
Q 
F 
3 
4 
PR 
F 
4 
B 
F 
4 
5 
6 
7 
8 
FLG 
JCFL 
DOPT 
I 
5 
H 
F 
5 
I 
6 
C 
F 
6 
I 
7 
8 
GAM0 
GAMM 
F 
7 
F 
8 
Variable 
A10 
A20 
A1H 
A2H 
A2S 
POW 
Type 
F 
  Card 4 
1 
F 
2 
Variable 
Type 
F 
F 
F 
F 
3 
D1 
F 
4 
D2 
F 
5 
D3 
F 
6 
D4 
F 
7 
8 
D1C 
D2C 
F
VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
FLG 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 𝜌. 
Young’s modulus 𝐸. 
Poisson’s ratio 𝜈. 
Flag to choose between yield functions 𝑓  and 𝑓 ̂, see Remarks. 
EQ.0.0: Cap in tension.  and Drucker & Prager in compression, 
EQ.2.0: Cap in tension.  and von Mises in compression. 
JCFL 
Johnson & Cook constitutive failure criterion flag, see Remarks. 
EQ.0.0: use triaxiality factor only in tension, 
EQ.1.0: use triaxiality factor in tension and compression. 
DOPT 
Damage criterion flag 𝐷̂  or 𝐷̌ , see Remarks. 
EQ.0.0: damage model uses damage plastic strain 𝑟, 
EQ.1.0: damage model uses plastic arc length 𝛾v. 
LCSS 
Curve ID or Table ID. 
If LCSS is a curve ID: 
The  curve  specifies  yield  stress  𝜏Y  as  a  function  of  plastic 
strain 𝑟. 
If LCSS is a Table ID: 
For  each  strain  rate  value  the  table  specifies  a  curve  ID
giving  the  yield  stress  versus  plastic  strain  for  that  strain
rate    or  it  defines  for  each  tempera-
ture  value  a  table  ID  which,  in  turn,  maps  strain  rates  to
curves giving the yield stress as a function of plastic strain
. 
The  yield  stress  versus  plastic  strain  curve  for  the  lowest
value of strain rate or temperature is used when the strain 
rate  or  temperature  falls  below  the  minimum  value.
Likewise,  maximum  values  cannot  be  exceeded.    Harden-
ing variables are ignored with this option (TAU0, Q, B, H,
C, GAM0, and GAMM).
*MAT_TOUGHENED_ADHESIVE_POLYMER 
DESCRIPTION
TAU0 
Initial shear yield stress 𝜏0. 
Q 
B 
H 
C 
Isotropic nonlinear hardening modulus 𝑞. 
Isotropic exponential decay parameter 𝑏. 
Isotropic linear hardening modulus 𝐻. 
Strain rate coefficient 𝐶. 
GAM0 
GAMM 
Quasi-static threshold strain rate 𝛾0. 
Maximum threshold strain rate 𝛾m. 
Yield function parameter: initial value 𝑎10 of 𝑎1 = 𝑎 ̂1(𝑟). 
Yield function parameter: initial value 𝑎20 of 𝑎2 = 𝑎 ̂2(𝑟). 
Yield function parameter 𝑎1
(ignored if FLG.EQ.2). 
H for formative hardening  
Yield function parameter 𝑎2
(ignored if FLG.EQ.2). 
H for formative hardening  
Plastic potential parameter 𝑎2
∗ for hydrostatic stress term. 
Exponent 𝑛 of the phenomenological damage model. 
Johnson & Cook failure parameter 𝑑1. 
Johnson & Cook failure parameter 𝑑2. 
Johnson & Cook failure parameter 𝑑3. 
Johnson & Cook rate dependent failure parameter 𝑑4. 
Johnson & Cook damage threshold parameter 𝑑1c. 
Johnson & Cook damage threshold parameter 𝑑2c. 
A10 
A20 
A1H 
A2H 
A2S 
POW 
D1 
D2 
D3 
D4 
D1C 
D2C 
Remarks: 
Two  different  𝐼1-𝐽2  yield  criteria  for  isotropic  plasticity  can  be  defined  by  parameter 
FLG:
Figure M252-1.  Yield function 𝑓  and plastic flow potential 𝑓 ∗ 
Figure M252-2.  Yield function 𝑓 ̂ and plastic flow potential 𝑓 ∗ 
1.  FLG = 0  is  used  for  the  yield  criterion  𝑓   which  is  changed  at  the  case  of 
hydrostatic pressure 𝐼1 = 0 into the Drucker & Prager model (DP) 
𝑓 ≔
𝐽2
(1 − 𝐷)2 +
√3
𝑎1𝜏0
𝐼1
1 − 𝐷
+
𝑎2
⟨
𝐼1
1 − 𝐷
⟩
− 𝜏Y
2 = 0 
with the Macauley bracket 〈∙〉,  the first invariant of the stress tensor 𝐼1 =  tr 𝛔, 
and  the  second  invariant  of  the  stress  deviator  𝐽2 = (1 2⁄ )tr(𝐬)2,  see  Figure 
M252-1.  
2.  FLG = 2 is used for the yield criterion 𝑓 ̂ which is changed at the vertex into the 
deviatoric  von  Mises  yield  function  –  see Figure  M252-2  –  and  is  used  for  con-
servative calculation in case of missing uniaxial compression or combined com-
pression and shear experiments: 
𝑓 ̂ ≔
𝐽2
(1 − 𝐷)2 +
𝑎2
⟨
𝐼1
1 − 𝐷
+
√3𝑎1𝜏0
2𝑎2
⟩
− (𝜏Y
2 +
2𝜏0
𝑎1
4𝑎2
) = 0 
The  yield  functions  𝑓   and  𝑓 ̂  are  formulated  in  terms  of  the  effective  stress  tensor 
  and  the  isotropic  material  damage  𝐷  according  to  the  continuum 
⁄
𝛔̃ = 𝛔 (1 − 𝐷)
Figure  M252-3.    Accumulated  plastic  strain  𝛾v  and  damage  plastic  strain  𝑟
versus strain 𝛾 
damage  mechanics  in  Lemaitre  [1992].    The  stress  tensor  𝛔  is  defined  in  terms  of  the 
elastic strain 𝛆e and the isotropic damage 𝐷: 
𝛔 = (1 − 𝐷)ℂ𝛆e 
The  continuity  (1 − 𝐷)  in  the  elastic  constitutive  equation  above  degrades  the  fourth 
order elastic stiffness tensor ℂ, 
ℂ = 2𝐺 (𝕀 −
𝟏⨂𝟏) + 𝐾 𝟏⨂𝟏 
with  shear  modulus  𝐺,  bulk  modulus  𝐾,  fourth  order  identity  tensor  𝕀,  and  second 
order  identity  tensor  𝟏.    The  plastic  strain  rate  𝛆̇p  is  given  by  the  non-associated  flow 
rule 
(1 − 𝐷)2 (𝐬 +
with the potential 𝑓 ∗ and an additional parameter 𝑎2
=
𝛆̇p = 𝜆
𝜕𝑓 ∗
𝜕𝛔
∗〈𝐼1〉𝟏) 
𝑎2
∗ < 𝑎2 to reduce plastic dilatancy. 
𝑓 ∗ ≔
𝐽2
(1 − 𝐷)2 +
∗
𝑎2
⟨
𝐼1
1 − 𝐷
⟩
2  
− 𝜏Y
The  plastic  arc  length  𝛾̇v  characterizes  the  inelastic  response  of  the  material  and  is 
defined by the Euclidean norm: 
𝛾̇v ≔ √2 tr(𝛆̇p)2 =
2𝜆
(1 − 𝐷)2
√𝐽2 +
(𝑎2
∗〈𝐼1〉)2 
In addition, the arc length of the damage plastic strain rate 𝑟 ̇ is introduced by means of 
the arc length 𝛾̇v and the continuity (1 − 𝐷) as in Lemaitre [1992], where 𝐼 ̃1 = 𝐼1 (1 − 𝐷)
and  𝐽 ̃2 = 𝐽2 (1 − 𝐷)2
⁄
 are the effective stress invariants, see Figure M252-3. 
⁄
𝑟 ̇ ≔ (1 − D)𝛾̇v = 2λ√𝐽 ̃2 +
∗⟨𝐼 ̃1⟩)
(𝑎2
The  rate-dependent  yield  strength  for  shear  𝜏Y  can  be  defined  by  two  alternative 
expressions.  The first representation is an analytic expression for 𝜏Y:
𝜏Y = (𝜏0 + 𝑅) [1 + 𝐶 (⟨ln
𝛾̇
𝛾̇0
⟩ − ⟨ln
𝛾̇
𝛾̇m
⟩)] ,  with  𝛾̇ = √2 tr(𝛆̇)2 
where the first factor (𝜏0 + 𝑅) in 𝜏Y is given by the static yield strength with the initial 
yield 𝜏0 and the non-linear hardening contribution  
𝑅 = 𝑞[1 − exp(−𝑏𝑟)] + 𝐻𝑟 
The  second  factor  [… ]  in  𝜏Y  describes  the  rate  dependency  of  the  yield  strength  by  a 
modified  Johnson  &  Cook  approach  with  the  reference  strain  rates  𝛾̇0  and  𝛾̇m  which 
Figure M252-4.  Rate-dependent tensile strength 𝜏Y versus effective strain rate
𝛾̇ (left) and effective damage plastic strain 𝑟 (right) 
limit the shear strength 𝜏Y, see Figure M252-4.  
The  second  representation  of  the  yield  strength  𝜏Y  is  the  table  definition  LCSS,  where 
hardening can be defined as a function of plastic strain, strain rate, and temperature. 
Toughened  structural  adhesives  show  distortional  hardening  under  plastic  flow,  i.e.  
the yield surface changes its shape.  This formative hardening can be phenomenological 
described by  simple evolution equations of parameters 𝑎1 = 𝑎 ̂1(𝑟)    ∧    𝑎2 = 𝑎 ̂2(𝑟) in the 
yield criterions 𝑓  with the initial values 𝑎10 and 𝑎20: 
H𝑟 ̇ 
𝑎1 = 𝑎 ̂1(𝑟) ∧ 𝑎 ̇1 = 𝑎1
𝑎2 = 𝑎 ̂2(𝑟) ∧ 𝑎2 ≥ 0 ∧ 𝑎 ̇2 = 𝑎2
H𝑟 ̇ 
H and 𝑎2
H can take positive or negative values as long as the inequality 
The parameters 𝑎1
𝑎2 ≥ 0  is  satisfied.    The  criterion  𝑎2 ≥ 0  ensures  an  elliptic  yield  surface.    The  yield 
criterion  𝑓 ̂  uses  only  the  initial  values  𝑎1 = 𝑎10  and  𝑎2 = 𝑎20  without  the  distortional 
hardening. 
The empirical  isotropic damage model  𝐷 is based on the approach  in Lemaitre [1985].  
Two  different  evolution  equations  𝐷̂̇ (𝑟, 𝑟 ̇)  and  𝐷̌̇ (𝛾v, 𝛾̇v)  are  available,  Figure  M252-5 
see.  The damage variable 𝐷 is formulated in  terms of the damage plastic strain rate 𝑟 ̇ 
(DOPT = 0) 
𝐷̇ = 𝐷̂̇ (𝑟, 𝑟 ̇) = 𝑛 ⟨
𝑛−1
𝑟 − 𝛾c
𝛾f − 𝛾c
⟩
𝑟 ̇
𝛾f − 𝛾c
Figure M252-5.  Influence of DOPT on damage softening 
or of the plastic arc length 𝛾̇v (DOPT = 1) 
𝐷̇ = 𝐷̌̇ (𝛾v, 𝛾̇v) = 𝑛 ⟨
𝑛−1
𝛾v − 𝛾c
𝛾f − 𝛾c
⟩
𝛾̇v
𝛾f − 𝛾c
where r in contrast to 𝛾v increases non-proportionally slowly, see Figure M252-5.  The 
strains at the thresholds 𝛾c and 𝛾f for damage initiation and rupture are functions of the 
triaxiality  𝑇 = 𝜎m 𝜎eq⁄
  with  the  hydrostatic  stress  𝜎m = 𝐼1 3⁄   and  the  von  Mises 
equivalent stress 𝜎eq = √3𝐽2 as in Johnson and Cook [1985]. 
𝛾c = [𝑑1c + 𝑑2cexp(−𝑑3〈𝑇〉)] (1 + 𝑑4 ⟨ln
⟩) 
𝛾f = [𝑑1 + 𝑑2exp(−𝑑3〈𝑇〉)] (1 + 𝑑4 ⟨ln
⟩) 
𝛾̇
𝛾̇0
𝛾̇
𝛾̇0
The  option  JCFL  controls  the  influence  of  triaxiality 𝑇 = 𝜎m 𝜎eq⁄
  in  the  pressure  range 
for  the  thresholds  𝛾c  and  𝛾f.    JCFL = 0  makes  use  of  the  Macauley  bracket  〈𝑇〉  for  the 
triaxiality 𝑇 = 𝜎m 𝜎eq⁄
 and JCFL = 1 omits the Macauley bracket 〈𝑇〉. 
History Variables: 
  VARIABLE   
DESCRIPTION
1 
2 
3 
4 
5 
6 
7 
damage variable 𝐷 
plastic arc length 𝛾v 
effective strain rate 
temperature 
yield stress 
damaged yield stress 
triaxiality
*MAT_GENERALIZED_PHASE_CHANGE 
This  is  Material  Type  254.    It  is  designed  to  model  phase  transformations  in  metallic 
materials  and  the  implied  changes  in  the  material  properties.    It  is  applicable  to  hot 
stamping,  heat  treatment  and  welding  processes  and  a  wide  range  of  steel  alloys.    It 
accounts  for  up  to  24  phases  and  provides  a  list  of  generic  phase  change  mechanisms 
for each possible phase changes.  The parameters for the phase transformation laws are 
to be given in tabulated form. 
Given  the  current  microstructure  composition,  the  material  formulation  implements  a 
temperature  and  strain-rate  dependent  elastic-plastic  material  with  non-linear 
hardening  behavior.    Above  a  certain  annealing  temperature,  the  material  behaves  as 
ideal elastic-plastic material with no evolution of plastic strains. 
So  far, the  material  has  been  implemented  for  solid  and  shell  elements  and  is  suitable 
for explicit and implicit analysis. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
N 
I 
3 
4 
YM 
F 
4 
5 
PR 
F 
5 
6 
7 
8 
MIX 
MIXR 
I 
6 
I 
7 
8 
Variable 
TASTRT 
TAEND 
CTE 
DTEMP 
TIME 
Type 
F 
  Card 3 
1 
F 
2 
I 
3 
4 
5 
6 
F 
7 
F 
8 
Variable 
PTLAW 
PTSTR 
PTEND 
PTX1 
PTX2 
PTX3 
PTX4 
PTX5 
Type 
I 
I 
I 
I 
I 
I 
I
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PTTAB1 
PTTAB2 
PTTAB3 
PTTAB4 
PTTAB5 
Type 
  Card 5 
I 
1 
I 
2 
I 
3 
I 
4 
I 
5 
6 
7 
8 
Variable 
PTEPS 
PTRIP 
Type 
I 
F 
GRAI 
F 
Phase Yield Stress Cards.  For each of the N phases, one parameter SIGYi has to be 
specified.  A keyword card (with a “*” in column 1) terminates this input if less than 10 
cards are used.  
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SIGY1 
SIGY2 
SIGY3 
SIGY4 
SIGY5 
SIGY6 
SIGY7 
SIGY8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
MID 
RO 
N 
YM 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 𝜌. 
Number of phases 
Youngs’ modulus: 
GT.0.0: constant value is used 
LT.0.0:  LCID or TABID.  Temperature dependent Youngs’ 
modulus  given  by  load  curve  ID = -E  or  a  Table 
ID = -E.    Use  TABID  to  describe  temperature  de-
pendent modulus for each phase individually.
VARIABLE   
DESCRIPTION
PR 
Poisson’s modulus: 
GT.0.0: constant value is used 
LT.0.0:  LCID  or  TABID. 
  Temperature  dependent 
Posson’s ratio given by load curve ID = -E or a Ta-
ble  ID = -E.    Use  TABID  to  describe  temperature 
dependent parameter for each phase individually. 
MIX 
MIXR 
Load curve ID with initial phase concentrations 
LCID  or  TABID  for  mixture  rule.    Use  a  TABID  to  define  a
temperature dependency 
TASTART 
TAEND 
Annealing temperature start
Annealing temperature end
CTE 
Coefficient of thermal expansion: 
GT.0.0: constant value is used 
LT.0.0:  LCID  or  TABID.    Temperature  dependent  CTE 
given  by  load  curve  ID = -CTE  or  a  Table  ID = -
CTE.    Use  Table  ID  to  describe  temperature  de-
pendent CTE for each phase individually. 
DTEMP 
TIME 
Maximum  temperature  variation  within  a  time  step.    If 
exceeded during the analysis a local sub-cycling is used 
Number  of  time  units  per  hour.    Default  is seconds,  that  is 
3600 time units per hour.
PTLAW 
PTSTR 
PTEND 
PTXi 
*MAT_GENERALIZED_PHASE_CHANGE 
DESCRIPTION
Table  ID  to  define    phase  transformation  model  as  a  function  of
source phase and target phase.  The   values  in *DEFINE_TABLE 
are the phase numbers before transformation (source phase).  The
curves  referenced  by  the  table  specify  transformation  model
(ordinate) versus phase number after transformation (abscissa). 
LT.0:  Transformation model used in cooling 
EQ.0:  No transformation 
GT.0:  Transformation model is used in heating 
There  are  four  possible  transformation  models  which  can  be
specified as ordinate values of the curves: 
EQ.1:  Koinstinen-Marburger 
EQ.2: 
JMAK 
EQ.3:  Akerstrom (only for cooling) 
EQ.4:   Oddy (only for heating) 
Table  ID  to  define  start  temperatures  for  the  transformations  as
function  of  source  phase  and  target  phase.    The    values  in 
*DEFINE_TABLE  are  the  phase  numbers  before  transformation 
(source  phase).    The  curves  referenced  by  the  table  specify  start
temperature (ordinate) versus phase number after transformation
(abscissa). 
Table  ID  to  define  end  temperatures  for  the  transformations  as
function  of  source  phase  and  target  phase.    The    values  in 
*DEFINE_TABLE  are  the  phase  numbers  before  transformation 
(source  phase).    The  curves  referenced  by  the  table  specify  end
temperature (ordinate) versus phase number after transformation
(abscissa). 
Table  ID  defining  the  i-th  scalar-valued  phase  transformation 
parameter  as  function  of  source  phase  and  target  phase  .  The  values in *DEFINE_TABLE are the phase 
numbers  before  transformation  (source  phase).    The  curves 
referenced by the table specify scalar parameter (ordinate) versus
phase number after transformation (abscissa).
VARIABLE   
PTTABi 
PTEPS 
PTRIP 
DESCRIPTION
i-th  tabulated  phase 
Table  ID  of  3D  table  defining  the 
transformation  parameter  as  function  of  source  phase  and  target 
phase  .    The    values  in  *DEFINE_TABLE_3D 
are the phase numbers before transformation (source phase).  The
values  in  the  2D  tables  referenced  by  *DEFINE_TABLE_3D  are 
the phase number after transformation.  The curves referenced by
the 2D tables specify tabulated parameter (ordinate) versus either
temperature or temperature rate (abscissa). 
Table ID containing transformation induced strains as function of 
source phase and target phase. 
Flag  for  transformation  induced  plasticity  (TRIP).    Algorithm
active for positive value of PTRIP. 
GRAIN 
Initial grain size. 
Remarks: 
This  material  features  temperature  and  phase  composition  dependent  elastic  plastic 
behavior.    The  phase  composition  is  determined  using  a  list  of  generic  phase 
transformation  mechanisms  the  user  can  choose  from  for  each  of  the  possible  phase 
transformations.   So  far,  four  different transformation  models  have  been  implemented 
to describe the transition from source phase 𝑥a to target phase 𝑥b: 
1.  Koistinen-Marburger:  
This  formulation  is  tailored  for    non-diffusive  transformations.    The  tempera-
ture dependent amount of the target phase is computed as 
The factor 𝛼 is to be defined in table PTX1. 
𝑥𝑏 = 𝑥𝑎(1.0 − 𝑒−𝛼(𝑇𝑠𝑡𝑎𝑟𝑡−𝑇)) 
2.  Generalized Johnson-Mehl-Avrami-Kolmogorov (JMAK): 
This widely used model employs the evolution equation 
𝑑𝑥𝑏
𝑑𝑡
= 𝑛(𝑇)(𝑘𝑎𝑏𝑥𝑎 − 𝑘𝑎𝑏
′ 𝑥𝑏)
for which the factors 
⎜⎛ln (
⎝
𝑘𝑎𝑏(𝑥𝑎 + 𝑥𝑏)
′ 𝑥𝑏
𝑘𝑎𝑏𝑥𝑎 − 𝑘𝑎𝑏
)
⎟⎞
⎠
𝑛(𝑇)−1.0
𝑛(𝑇)
𝑘𝑎𝑏 =
𝑥𝑒𝑞(𝑇)
𝜏(𝑇)
𝑓 (𝑇̇), 𝑘𝑎𝑏
′ =
1.0 − 𝑥𝑒𝑞(𝑇)
𝜏(𝑇)
𝑓 ′(𝑇̇) 
have to be defined.  
As user input, load curve data for the exponent 𝑛(𝑇) in PTTAB1, the equilibri-
um concentration 𝑥𝑒𝑞(𝑇) in PTTAB2, the relaxation time 𝜏(𝑇)  in PTTAB3, and
the temperature rate correction factors 𝑓 (𝑇̇) and 𝑓′(𝑇̇) in PTTAB4 and PTTAB5, 
respectively, are expected. 
3.  Kirkaldy: 
Similar  to  the  implementation  of  *MAT_244,    the  transformation  for  cooling 
phases can be computed by the evolution equation  
𝑑𝑋𝑏
𝑑𝑡
= 20.5(𝐺−1)𝑓 (𝐶)(𝑇𝑠𝑡𝑎𝑟𝑡 − 𝑇)𝑛𝑇𝐷(𝑇)
𝑋𝑏
𝑛1(1.0−𝑋𝑏)(1.0 − 𝑋𝑏)𝑛2𝑋𝑏
Y(𝑋𝑏)
𝑥𝑏
. 
𝑥𝑒𝑞(𝑇)
formulated in the normalized phase concentration 𝑋𝑏 =
In  contrast  to  *MAT_244,  the  parameters  for  the  evolution  equation  are  not 
determined from the chemical composition of the material but defined directly 
as user input.   The  scalar data in PTX1 to PTX4 are interpreted as 𝑓 (𝐶), 𝑛𝑇, 𝑛1, 
and  𝑛2.    Tabulated  data  for  𝐷(𝑇), 𝑌(𝑋𝑏),  and  𝑥𝑒𝑞(𝑇)  are  given  in  PTTAB1  to 
PTTAB3. 
4.  Oddy: 
For phase transformation in heating, the equation of Oddy can be used, which 
can be interpreted as a simplified JAMK relation and  reads 
𝑑𝑥𝑏
𝑑𝑡
= 𝑛
𝑥𝑎
𝑐1(𝑇 − 𝑇𝑠𝑡𝑎𝑟𝑡)−𝑐2 ⎝
⎜⎛ln (
(𝑥𝑎 + 𝑥𝑏)
𝑥𝑎
⎟⎞
)
⎠
𝑛−1.0
Its application requires the input of three scalar parameters 𝑛, 𝑐1, 𝑐2 that are read 
from the respective positions in the tables in PTX1 to PTX3.
*MAT_PIECEWISE_LINEAR_PLASTIC_THERMAL 
This is material type 255, an isotropic elastoplastic material with thermal properties.  It 
can  be  used  for  both  explicit  and  implicit  analyses.    Young’s  modulus  and  Poisson’s 
ratio can depend on the temperature by defining two load curves.  Moreover, the yield 
stress in tension and compression are given as load curves for different temperatures by 
using  two  tables.    The  thermal  coefficient  of  expansion  can  be  given  as  a  constant 
ALPHA or as a load curve, see LALPHA at position 3 on card 2.  A positive curve ID for 
LALPHA  models  the  instantaneous  thermal  coefficient,  whereas  a  negatives  curve  ID 
models the thermal coefficient relative to a reference temperature, TREF.  The strain rate 
effects are modelled with the Cowper-Symonds rate model with the parameters C and P 
on  card  1.    Failure  can  be  based  on  effective  plastic  strain  or  using  the  *MAT_ADD_-
EROSION keyword. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
E 
F 
3 
Variable 
TABIDC 
TABIDT 
LALPHA 
Type 
I 
  Card 3 
1 
I 
2 
I 
3 
Variable 
ALPHA 
TREF 
Type 
F 
F 
4 
PR 
F 
4 
4 
5 
C 
F 
5 
VP 
F 
5 
6 
P 
F 
6 
7 
8 
FAIL 
TDEL 
F 
7 
F 
8 
6 
7 
8 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density.
*MAT_PIECEWISE_LINEAR_PLASTIC_THERMAL 
DESCRIPTION
E 
Young’s modulus: 
LT.0.0:  E  is  given  as  a  function  of  temperature,  T.    The  curve
consists  of  (T,E)  data  pairs.    Enter  |E|  on  the  DE-
FINE_CURVE keyword. 
GT.0.0:  E is constant. 
PR 
Poisson’s ratio. 
LT.0.0:  |PR|  is  the  LCID  for  Poisson’s  ratio  versus  tempera-
C 
P 
FAIL 
TDEL 
ture. 
GT.0.0:  PR is constant 
Strain rate parameter.  See Remark 1. 
Strain rate parameter.  See Remark 1. 
Effective  plastic  strain  when  the  material  fails.    User  defined
failure  subroutine,  matusr_24  in  dyn21.F,  is  called  to  determine 
failure  when  FAIL < 0.    Note  that  for  solids  the  *MAT_ADD_-
EROSION can be used for additional failure criteria. 
A time step less than TDEL is not allowed.  A step size less than
TDEL trigger automatic element deletion.  This option is ignored
for implicit analyses. 
TABIDC 
Table ID for yield stress in compression, see Remark 2. 
TABIDT 
Table ID for yield stress in tension, see Remark 2. 
LALPHA 
Load  curve  ID  for  thermal  expansion  coefficient  as  a  function  of
temperature. 
GT.0.0:  the  instantaneous  thermal  expansion  coefficient  based
on the following formula: 
𝑑𝜀𝑖𝑗
thermal = 𝛼(𝑇)𝑑𝑇𝛿𝑖𝑗 
LT.0.0:  the  thermal  coefficient  is  defined  relative  a  reference
temperature TREF, such that the total thermal strain is
given by: 
thermal = 𝛼(𝑇)(𝑇 − 𝑇ref)𝛿𝑖𝑗 
𝜀𝑖𝑗
With this option active, ALPHA is ignored.
VARIABLE   
DESCRIPTION
VP 
Formulation for rate effects, see Remarks 1 and 2. 
EQ.0.0: effective total strain rate (default) 
NE.0.0:  effective plastic strain rate 
ALPHA 
Coefficient of thermal expansion 
TREF 
Reference temperature, which is required if and only if LALPHA
is given with a negative load curve ID. 
Remarks: 
1.  Strain  Rate  Effects.    The  strain  rate  effect  is  modelled  by  using  the  Cowper 
and Symonds model which scales the yield stress according to the factor 
1 + (
𝜀̇eff
1 𝑃⁄
)
where  𝜀̇eff = √tr(𝛆̇𝛆̇T)  is  the  Euclidean  norm  of  the  total  strain  rate  tensor  if 
𝑝 . 
VP = 0 (default), otherwise 𝜀̇eff = 𝜀̇eff
2.  Yield  Stress  Tables.  The  dependence  of  the  yield  stresses  on  the  effective 
plastic strains is given in two tables. 
a)  TABIDC gives the behaviour of the yield stresses in compression 
b)  TABIDT gives the behaviour of the yield stresses in tension. 
The table indices consist of temperatures, and at each temperature a yield stress 
curve must be defined. 
Both TABIDC and TABIDT can be 3D tables, in which temperatures indexes the 
main table and strain rates are defined as values for the sub tables with harden-
ing  curves  as  targets  for  those  strain  rates.  If  the  same  yield  stress  should  be 
used in both tension and compression, only one table needs to be defined and 
the same TABID is put in position 1 and 2 on card 2.  If VP = 0, effective total 
strain rates are used in the 3D tables, otherwise plastic strain rates. 
3.  History  Variables.    Two  history  variables  are  added  to  the  d3plot  file,  the 
Young’s modulus and the Poisson’s ratio, respectively.  They can be requested 
through the *DATABASE_EXTENT_BINARY keyword.
4.  Nodal  Temperatures.    Nodal  temperatures  must  be  defined  by  using  a 
coupled  analysis  or  some  other  way  to  define  the  temperatures,  such  as 
*LOAD_THERMAL_VARIABLE or *LOAD_THERMAL_LOAD_CURVE.
*MAT_AMORPHOUS_SOLIDS_FINITE_STRAIN 
This  is  material  type  256,  an  isotropic  elastic-viscoplastic  material  model  intended  to 
describe  the  behaviour  of  amorphous  solids  such  as  polymeric  glasses.    The  model 
accurately  captures  the  hardening-softening-hardening  sequence  and  the  Bauschinger 
effect  experimentally  observed  at  tensile  loading  and  unloading  respectively.    The 
formulation  is  based  on  hyperelasticity  and  uses  the  multiplicative  split  of  the 
deformation  gradient  F  which  makes  it  naturally  suitable  for  both  large  rotations  and 
large strains.  Stress computations are performed in an intermediate configuration and 
are therefore preceded by a pull-back and followed by a push-forward.  The model was 
originally developed by Anand and Gurtin [2003] and implemented for solid elements 
by Bonnaud and Faleskog [2008] 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
  Card 2 
1 
Variable 
ALPHA 
Type 
F 
2 
H0 
F 
3 
K 
F 
3 
SCV 
F 
4 
G 
F 
4 
B 
F 
5 
MR 
F 
5 
ECV 
F 
6 
LL 
F 
6 
G0 
F 
7 
NU0 
F 
7 
S0 
F 
8 
M 
F 
8 
  VARIABLE   
DESCRIPTION
MID 
RO 
K 
G 
MR 
LL 
NU0 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
Bulk modulus 
Shear modulus 
Kinematic hardening parameter: μR  
Kinematic hardening parameter: λL  
Creep parameter:  ν0
*MAT_AMORPHOUS_SOLIDS_FINITE_STRAIN 
DESCRIPTION
M 
ALPHA 
Creep parameter: m  
Creep parameter: α  
Isotropic hardening parameter: h0  
Isotropic hardening parameter: scv  
Isotropic hardening parameter: b  
Isotropic hardening parameter: ηcv  
Isotropic hardening parameter: g0  
Isotropic hardening parameter: s0  
H0 
SCV 
B 
ECV 
G0 
S0 
Remarks: 
1.  Kinematic  hardening  gives  rise  to  the  second  hardening  occurrence  in  the 
hardening-softening-hardening  sequence.    The  constants  μR  and  λL  enter  the 
back stress μB  (where B is the left Cauchy-Green deformation tensor) through 
the function μ according to: 
𝜇 = 𝜇𝑟 (
𝜆𝐿
3𝜆𝑝) 𝐿−1 (
𝜆𝑝
𝜆𝐿
)
(256.1)
Where  𝜆𝑝 = 1
√3
√𝑡𝑟(𝐵𝑝)  and  𝐵𝑝  is  the  plastic  part  of  the  left  Cauchy-Green  de-
formation tensor and where L is the Langevin function defined by, 
𝐿(𝑋) = coth(𝑋) − 𝑋−1 
2.  This material model assumes plastic incompressibility.  Nevertheless in order to 
account  for  the  different  behaviours  in  tension  and  compression  a  Drucker-
Prager law is included in the creep law according to: 
𝜈𝑝 = 𝜈0 (
𝜏̅
𝑠 + 𝛼𝜋
𝑚⁄
)
(256.2)
Where  𝜈𝑝  is  the  equivalent  plastic  shear  strain  rate, 
stress, s the internal variable defined below and -π the hydrostatic stress. 
the  equivalent  shear 
3. 
Isotropic  hardening  gives  rise  to  the  first  hardening  occurrence  in  the  harden-
ing-softening-hardening sequence.  Two coupled internal variables are defined:
s  the  resistance  to  plastic  flow  and  η  the  local  free  volume.    Their  evolution 
equations read: 
𝑠 ̇ = ℎ0 [1 −
𝑠 ̃(𝜂)
] 𝜈𝑝
𝜂̇ = 𝑔0 (
𝑠𝑐𝑣
− 1) 𝜈𝑝
𝑠 ̃(𝜂) = 𝑠𝑐𝑣[1 + 𝑏(𝜂𝑐𝑣 − 𝜂)]
(256.3)
(256.4)
(256.5)
4.  Typical material parameters values are given in Ref.1 for Polycarbonate: 
  PolyC 1 
1 
Variable 
MID 
Value 
  PolyC 2 
1 
Variable 
ALPHA 
2 
RO 
2 
H0 
3 
K 
4 
G 
5 
MR 
6 
LL 
7 
NU0 
8 
M 
2.24GPa  0.857GPa 11.0MPa 
1.45 
0.0017s-1 
0.011 
3 
SCV 
4 
B 
5 
ECV 
6 
G0 
7 
S0 
8 
Value 
0.08 
2.75GPa  24.0MPa 
825 
0.001 
0.006 
20.0MPa 
[1]  Anand,  L.,  Gurtin,  M.E.,  2003,  “A  theory  of  amorphous  solids  undergoing  large 
deformations,  with  application  to  polymeric  glasses,”  International  Journal  of  Solids  and 
Structures, 40, pp.  1465-1487.
*MAT_STOUGHTON_NON_ASSOCIATED_FLOW 
This  is  Material  Type  260A.    This  material  model  is  implemented  based  on  non-
associated  flow  rule  models  (Stoughton  2002  and  2004).    Strain  rate  sensitivity  can  be 
included using a load curve.  This model applies to both shell and solid elements. 
Available options include: 
<BLANK> 
XUE 
The option XUE is available for solid elements only.   
Card 1 
1 
2 
Variable 
MID 
RO 
Type 
A8 
F 
3 
E 
F 
4 
5 
6 
7 
8 
PR 
R00 
R45 
R90 
SIG00 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SIG45 
SIG90 
SIG_B 
LCIDS 
LCIDV 
SCALE 
Type 
F 
F 
F 
I 
I 
F 
Default 
none 
none 
none 
none 
none 
1.0 
Define the following card only for the option XUE (available for solids only):
6 
7 
8 
Card 3 
1 
2 
Variable 
EF0 
PLIM 
Type 
F 
F 
3 
Q 
F 
4 
GAMA 
F 
5 
M 
F 
Default 
none 
none 
none 
none 
none 
Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
AOPT 
Type 
F 
Default 
none 
Card 4 
1 
Variable 
XP 
Type 
F 
2 
YP 
F 
3 
ZP 
F 
4 
A1 
F 
5 
A2 
F 
6 
A3 
F 
7 
8 
Default 
none 
none 
none 
none 
none 
none
Card 5 
1 
Variable 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
5 
6 
7 
8 
D1 
D2 
D3 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s Modulus 
Poisson’s ratio 
R00, R45, 
R90 
Lankford parameters in rolling (0°), diagonal (45°) and transverse 
(90°) directions, respectively; determined from experiments. 
SIG00, 
SIG45, 
SIG90, SIG_B 
SIG00: the initial yield stress from uniaxial tension tests in rolling 
(0°) direction;  
SIG45:  the  initial  yield  stress  from  uniaxial  tension  tests  in 
diagonal (45°) direction; 
SIG90:  the  initial  yield  stress  from  uniaxial  tension  tests  in 
transverse (90°) directions; 
SIG_B: the initial yield stress from equi-biaxial stretching tests. 
LCIDS 
ID  of  a  load  curve  defining  stress  vs.    strain  hardening  behavior
from a uniaxial tension test along the rolling direction.
VARIABLE   
LCIDV 
SCALE 
DESCRIPTION
ID  of  a  load  curve  defining  stress  scale  factors  vs.    strain  rates; 
determined  from  experiments.    An  example  of  the  curve  can  be
found in Figure M260A-2.  Furthermore, strain rates are stored in 
history variable #5.  Strain rate scale factors are stored in history
variable #6.  To turn on the variables for viewing in LS-PrePost, set 
NEIPS  to  at  least  “6”  in  *DATABASE_EXTENT_BINARY.    It  is 
very  useful  to  know  what  levels  of  strain  rates,  and  strain  rate
scale  factors  in  a  particular  simulation.    Once  d3plot  files  are 
opened  in  LS-PrePost,  individual  element  time  history  can  be 
plotted via menu option Post → History, or a color contour of the 
entire  part  can  be  viewed  with  the  menu  option  Post  →  FriComp
→ Misc. 
This  variable  can  be  used  to  speed  up  the  simulation  while
equalizing  the  strain  rate  effect,  useful  especially  in  cases  where
the  pulling  speed  or  punch  speed  is  slow.    For  example,  if  the
pulling  speed  is  at  15  mm/s  but  running  the  simulation  at  this
speed will take a long time, the pulling speed can be increased to
500  mm/s  while  "SCALE"  can  be  set  to  0.03,  giving  the  same
results  as  those  from  15  mm/s,  but  with  the  benefit  of  greatly
reduced computational time, see Figures M260A-3 and M260A-4. 
Note  the  increased  absolute  value  (within  a  reasonable  range) of
mass  scaling  -1.0*dt2ms  frequently  used  in  forming  simulation 
does not affect the strain rates, as shown in the Figure M260A-5. 
EF0, PLIM, 
Q, GAMA, 
M 
Material parameters for the option XUE.  The parameter k in the 
original paper is assumed to be 1.0.   For details, refer to Xue, L.,
Wierzbicki,  T.’s  2009  paper  “Numerical  simulation  of  fracture  mode 
transition  in  ductile  plates”  in  the  International  Journal  of  Solids  and 
Structures.
AOPT 
*MAT_STOUGHTON_NON_ASSOCIATED_FLOW 
DESCRIPTION
Material axes option : 
EQ.0.0:  locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES,  and  then  rotated  about  the  shell  ele-
ment normal by the angle BETA. 
EQ.1.0:  locally  orthotropic  with  material  axes  determined  by 
the point 𝐩 in space and the global location of the ele-
ment  center;  this  is  the  𝐚-direction.    This  option  is  for 
solid elements only. 
EQ.2.0:  globally  orthotropic  with  material  axes  determined  by
the vector 𝐚 for shells and by both vectors 𝐚 and 𝐝 for 
solids, as with *DEFINE_COORDINATE_VECTOR. 
EQ.3.0:  locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  𝐯  with  the 
element  normal.    The  plane  of  a  solid  element  is  the 
mid-surface  between  the  inner  surface  and  outer  sur-
face  defined  by  the  first  four  nodes  and  the  last  four
nodes of the connectivity of the element, respectively. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE__CO-
ORDINATE_VECTOR). 
XP, YP, ZP 
Coordinates of point 𝐩 for AOPT = 1. 
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2, for shells and solids. 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3. 
D1, D2, D3 
Components of vector 𝐝 for AOPT = 2, for solids. 
The Stoughton non-associated flow rule: 
In  non-associated  flow  rule,  material  yield  function  does  not  equal  to  the  plastic  flow 
potential.  According to Thomas B.  Stoughton’s paper titled “A non-associated flow rule 
for  sheet  metal  forming”  in  2002  International  Journal  of  Plasticity  18,  687-714,  and  “A 
pressure-sensitive  yield  criterion  under  a  non-associated  flow  rule  for  sheet  metal  forming”  in 
2004 International Journal of Plasticity 20, 705-731, plastic potential is defined by:
𝜎̅̅̅̅̅𝑝 = √𝜎11
2 + 𝜆𝑝𝜎22
2 − 2𝜈𝑝𝜎11𝜎22 + 2𝜌𝑝𝜎12
where 𝜎𝑖𝑗 is the stress tensor component; where also, 
𝜆𝑝   =
1 + 1
𝑟90
1 + 1
𝑟0
, 
, 
𝜈𝑝   =
𝑟0
1 + 𝑟0
+ 1
𝑟0
𝑟90
1 + 1
𝑟0
where 𝑟0, 𝑟45,  𝑟90 are Lankford parameters in the rolling (0°), the diagonal (45°) and the 
transverse (90°) directions, respectively. 
+ 𝑟45). 
𝜌𝑝   =
(
Yield function is defined by: 
𝜎̅̅̅̅̅𝑦 = √𝜎11
2 + 𝜆𝑦𝜎22
2 − 2𝜈𝑦𝜎11𝜎22 + 2𝜌𝑦𝜎12
where, 
𝜆𝑦   = (
𝜎0
𝜎90
)
, 
𝜈𝑦   =
𝜌𝑦   =
[1 + 𝜆𝑦 − (
)
𝜎0
𝜎𝑏
] , 
[(
)
2𝜎0
𝜎45
− (
𝜎0
𝜎𝑏
)
]. 
where 𝜎0, 𝜎45, 𝜎90 are the initial yield stresses from uniaxial tension tests in the rolling 
(0°), the diagonal (45°), and the transverse (90°) directions, respectively.  𝜎𝑏 is the initial 
yield stress from an equi-biaxial stretching test. 
The  required  stress-strain  hardening  curve  must  be  for  uniaxial  tension  along  the 
rolling  direction.    Strain  rate  sensitivity  is  implemented  as  an  option,  by  defining  a 
curve (LCIDV) of strain rates vs.  stress scale factors, see Figure M260A-2. 
The variable SCALE is very useful in speeding up the simulation while equalizing the 
strain  rate  effect.    For  example,  if  the  real,  physical  pulling  speed  is  at  15  mm/s  but 
running at this speed will take a long time, one could increase the pulling speed to 500 
mm/s  while  setting  the  SCALE  to  0.03,  resulting  in  the  same  results  as  those  from  15
mm/s  with  the  benefit  of  greatly  reduced  computational  time.    See  examples  in 
Verification. 
History variables: 
1.  Strain rates: history variable #5. 
2.  Strain rate scale factors: history variable #6. 
Verification: 
Uniaxial tension tests were done on a single shell element as shown in Figure M260A-1.  
Strain  rate  effect  LCIDV  is  input  as  shown  in  Figure  M260A-2.    In  Figure  M260A-3, 
pulling  stress  vs.    strain  from  various  test  conditions  are  compared  with  input  stress-
strain  curve  A.    In  summary,  using  the  parameter  SCALE,  the  element  can  be  pulled 
much faster (500 mm/s vs.  15 mm/s) but achieve the same stress vs.  strain results, the 
same  strain  rates  (history  variable  #5),  and  the  same  strain  rate  scale  factor  (history 
variable  #6  in  Figure  M260A-4).    Simulation  speed  can  be  improved  further  with 
increased mass scaling (-1.0*dt2ms) without affecting the results, see Figure M260A-5. 
A  partial  keyword  input  is  provided  below,  for  the  case  with  pulling  speed  of  500 
mm/s,  strain  hardening  curve ID of  100,  LCIDV  curve  ID  of  105,  and  strain  rate  scale 
factor of 0.03. 
*KEYWORD 
*parameter_expression 
R endtime     0.012 
R v           500.0 
*CONTROL_TERMINATION 
$   ENDTIM    ENDCYC     DTMIN    ENDNEG    ENDMAS 
&endtime 
*MAT_STOUGHTON_NON_ASSOCIATED_FLOW 
$#     mid        Ro         E        PR       R00       R45       R90     SIG00 
         1 7.8000E-9   2.10E05  0.300000       1.1       1.2       1.3     150.4 
$    SIG45     SIG90     SIG_B     LCIDS     LCIDV     SCALE 
     150.1     150.2    150.30       100       105      0.03 
$     AOPT       
         3 
$       XP        YP        ZP        A1        A2        A3 
$       V1        V2        V3        D1        D2        D3      BETA 
                 1.0 
*DEFINE_CURVE 
       100 
         0.00000E+00         0.30130E+03 
         0.10000E-01         0.42295E+03 
         0.20000E-01         0.47991E+03 
         0.30000E-01         0.52022E+03 
         0.40000E-01         0.55126E+03 
         0.50000E-01         0.57615E+03 
⋮ 
*DEFINE_CURVE 
2-1298 (MAT_248)
105 
         0.00000E+00         0.10000E+01 
         0.10000E+00         0.10608E+01 
         0.50000E+00         0.10828E+01 
         0.10000E+01         0.10923E+01 
*END 
⋮ 
⋮ 
Revision information: 
This material model is available starting in Revision 101821 in explicit, SMP only.  The 
option XUE is available starting on Revision 112711.
Fy
0=
n i- a
x i a l str e s s
Fy
0=
n str a i n
e ll
 s h
Figure M260A-1.  Uniaxial tension tests on a single shell element. 
1.2
1.15
1.1
1.05
1.0
0.0
LCIDV
1.5
2.0
0.5
1.0
Strain rate (x103)
Figure M260A-2.  Input LCIDV.
1000
800
600
400
200
)
(
Input
Pull speed: 15 mm/s,
no LCIDV, SCALE=1.0
Pull speed: 15 mm/s,
LCIDV, SCALE=1.0
Pull speed: 500 mm/s,
LCIDV, SCALE=1.0
Pull speed: 500 mm/s,
LCIDV, SCALE=0.03
0.0
0.2
0.4
0.6
0.8
1.0
Strain
)
/
(
-
#
3.5
3.0
2.5
2.0
1.5
1.0
0.5
0.0
0.03
0.06
0.09
Pull speed: 15 mm/s,
LCIDV, SCALE=1.0
Pull speed: 500 mm/s,
LCIDV, SCALE=1.0
Pull speed: 500 mm/s,
LCIDV, SCALE=0.03
0.1
0.2
Time (sec)
0.3
0.012
100
86
72
58
44
30
15
0.4
Figure M260A-3.  Recovered stress-strain curve (top) and strain rates (bottom)
under various conditions shown.
1.12
1.1
1.08
1.06
1.04
1.02
-
#
1.00
0.0
0.03
0.06
0.09
0.012
1.16
Pull speed: 15 mm/s,
LCIDV, SCALE=1.0
Pull speed: 500 mm/s,
LCIDV, SCALE=1.0
Pull speed: 500 mm/s,
LCIDV, SCALE=0.03
0.1
0.2
Time (sec)
0.3
1.13
1.11
1.08
1.05
1.03
1.00
0.4
Figure M260A-4.  Recovered strain rate scale factors under various conditions
shown. 
1000
800
600
400
200
)
(
Input
Pull speed: 500 mm/s,
LCIDV, SCALE=0.03, DT2MS=0.0
Pull speed: 500 mm/s,
LCIDV, SCALE=0.03, DT2MS=-4E-6
0.0
0.2
0.4
0.6
0.8
1.0
Figure M260A-5.  Effect of mass scaling (-1.0*dt2ms). 
Strain
*MAT_MOHR_NON_ASSOCIATED_FLOW_{OPTION} 
This is Material Type 260B.  This material model is implemented based on the papers by 
Mohr,  D.,  et  al.(2010)  and  Roth,  C.C.,  Mohr,  D.  (2014).    The  Johnson-Cook  plasticity 
model  of  strain  hardening,  strain  rate  hardening,  and  temperature  soften  effect  is 
modified  with  a  mixed  Swift-Voce  strain  hardening  function,  coupled  with  a  non-
associated flow rule which accounts for the difference between directional dependency 
of  the  𝑟-values  (planar  anisotropic),  and  planar  isotropic  material  response  of  certain 
Advanced High Strength Steels (AHSS).  A ductile fracture model is included based on 
Hosford-Coulomb fracture initiation model.  This model applies to shell elements only. 
Available options include: 
<BLANK> 
XUE 
Card 1 
1 
2 
Variable 
MID 
RO 
Type 
A8 
F 
3 
E 
F 
4 
5 
6 
7 
8 
PR 
P12 
P22 
P33 
G12 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
G22 
G33 
LCIDS 
LCIDV 
LCIDT 
LFLD 
LFRAC 
W0 
Type 
F 
F 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
I 
0 
I 
F 
none 
none
Card 3 
Variable 
Type 
1 
A 
F 
2 
3 
B0 
GAMMA 
F 
F 
4 
C 
F 
5 
N 
F 
6 
7 
8 
SCALE 
SIZE0 
F 
F 
Default 
none 
none 
none 
none 
none 
1.0 
none 
Card 4 
1 
2 
Variable 
TREF 
TMELT 
Type 
F 
F 
3 
M 
F 
4 
5 
6 
7 
8 
ETA 
CP 
TINI 
DEPSO 
DEPSAD 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Define the following card only for the option XUE: 
Card 5 
1 
2 
Variable 
EF0 
PLIM 
Type 
F 
F 
3 
Q 
F 
4 
GAMA 
F 
5 
M 
F 
Default 
none 
none 
none 
none 
none 
6 
7
Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
AOPT 
Type 
F 
Default 
none 
Card 6 
1 
2 
3 
Variable 
Type 
Default 
Card 7 
1 
Variable 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
Default 
none 
none 
none 
7 
8 
4 
A1 
F 
5 
A2 
F 
6 
A3 
F 
none 
none 
none 
4 
5 
6 
7 
8 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s Modulus 
Poisson’s ratio
P12, P22, P33 
G12, G22, 
G33 
LCIDS 
LCIDV 
LCIDT 
LFLD 
LFRAC 
*MAT_MOHR_NON_ASSOCIATED_FLOW 
DESCRIPTION
Yield  function  parameters,  defined  by  Lankford  parameters  in
rolling  (0°),  diagonal  (45°)  and  transverse  (90°)  directions, 
respectively; see Non-associated flow rule. 
Plastic 
flow  potential  parameters,  defined  by  Lankford
parameters  in  rolling  (0°),  diagonal  (45°)  and  transverse  (90°) 
directions, respectively; see Non-associated flow rule. 
Load curve ID defining stress vs.  strain hardening behavior from
a  uniaxial  tension  test;  must  be  along  the  rolling  direction.    Also 
see A modified Johnson-Cook. 
Load curve ID defining stress scale factors vs.  strain rates (Figure 
M260B-1 middle); determined from experiments.  Strain rates are 
stored in history variable #5.  Strain rate scale factors are stored in 
history  variable  #6.    To  turn  on  the  variables  for  viewing  in  LS-
PrePost,  set  NEIPS  to  at  least  “6”  in  *DATABASE_EXTENT_BI-
NARY.  It is very useful to know what levels of strain rates, and 
strain  rate  scale  factors  in  a  particular  simulation.    Once  d3plot
files are opened in LS-PrePost, individual element time history can 
be  plotted  via  menu  option  Post  →  History,  or  a  color  contour  of 
the  entire  part  can  be  viewed  with  the  menu  option  Post  → 
FriComp → Misc.  Also see A modified Johnson-Cook. 
Load  curve  ID  defining  stress  scale  factors  vs.    temperature  in
Kelvin  (Figure  M260B-1  bottom);  determined  from  experiments. 
Temperatures  are  stored  in  history  variable  #4.    Temperature
scale  factors  are  stored  in  history  variable  #7.    To  turn  on  this
variable  for  viewing  in  LS-PrePost,  set  NEIPS  to  at  least  “7”  in 
*DATABASE_EXTENT_BINARY.  It is very useful to know what
levels  of  temperatures  and  temperature  scale  factors  in  a
particular simulation.  Once d3plot files are opened in LS-PrePost, 
individual  element  time  history  can  be  plotted  via  menu  option 
Post → History, or a color contour of the entire part can be viewed
with  the  menu  option  Post  →  FriComp  →  Misc.    Also  see  A 
modified Johnson-Cook. 
Load  curve  ID  defining  traditional  Forming  Limit  Diagram  for
linear strain paths. 
Load  curve  ID  defining  a  fracture  limit  curve.    Leave  this  field
empty if parameters A, B0, GAMMA, C, N are defined.  However,
if  this  field  is  defined,  parameters  A,  B0,  GAMMA,  C,  N  will  be
ignored even if they are defined.
VARIABLE   
DESCRIPTION
W0 
Neck (FLD failure) width, typically is the blank thickness. 
A, B0, 
GAMMA, C, 
N 
SCALE 
Material  parameters  for  the  rate-dependent  Hosford-Coulomb 
fracture initiation model, see Rate-dependent Hosford-Coulomb. 
This  variable  can  be  used  to  speed  up  the  simulation  while
equalizing  the  strain  rate  effect,  useful  especially  in  cases  where
the  pulling  speed  or  punch  speed  is  slow.    For  example,  if  the
pulling  speed  is  at  15  mm/s  but  running  the  simulation  at  this
speed will take a long time, the pulling speed can be increased to
500  mm/s  while  "SCALE"  can  be  set  to  0.03,  giving  the  same
results  as  those  from  15  mm/s,  but  with  the  benefit  of  greatly
reduced  computational  time,  see  examples  and  Figures  in 
*MAT_260A  for  details.    Furthermore,  the  increased  absolute 
value  (within  a  reasonable  range)  of  mass  scaling  -1.0*dt2ms
frequently  used  in  forming  simulation  does  not  affect  the  strain
rates, as shown in the examples and Figures in *MAT_260A. 
SIZE0 
Fracture  gage  length  used  in  an  experimental  measurement, 
typically between 0.2~0.5mm. 
TREF, 
TMELT, M, 
ETA, CP, 
TINI, DEPS0, 
DEPSAD 
EF0, PLIM, 
Q, GAMA, 
M 
Material  parameters 
to
strain 
temperature.    TINI  is  the  initial  temperature.    See  A  modified 
Johnson-Cook for other parameters’ definitions. 
softening  effect  due 
for 
Material parameters for the option XUE.  The parameter k in the 
original paper is assumed to be 1.0.   For details, refer to Xue, L.,
Wierzbicki,  T.’s  2009  paper  “Numerical  simulation  of  fracture  mode 
transition  in  ductile  plates”  in  the  International  Journal  of  Solids  and 
Structures.
AOPT 
*MAT_MOHR_NON_ASSOCIATED_FLOW 
DESCRIPTION
Material axes option : 
EQ.0.0: 
EQ.2.0: 
EQ.3.0: 
LT.0.0: 
locally  orthotropic  with  material  axes  determined 
by  element  nodes  1,  2,  and  4,  as  with  *DEFINE_-
COORDINATE_NODES,  and  then  rotated  about 
the shell element normal by the angle BETA. 
globally orthotropic with material axes determined
by the vector 𝐚 for shells, as with *DEFINE_COOR-
DINATE_VECTOR. 
locally  orthotropic  material  axes  determined  by
rotating  the  material  axes  about  the  element  nor-
mal by an angle, BETA, from a line in the plane of
the  element  defined  by  the  cross  product  of  the
vector 𝐯 with the element normal. 
the absolute value of AOPT is a coordinate system
ID  number  (CID  on  *DEFINE_COORDINATE_-
NODES, 
*DEFINE_COORDINATE_SYSTEM  or 
*DEFINE__COORDINATE_VECTOR). 
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3. 
Non-associated flow rule: 
Referring  to  Mohr,  D.,  Dunand,  M.,  and  Kim,  K-H.’s  2010  and  2014  papers  in  the 
International Journal of Plasticity, Hill’s 1948 quadratic yield function is written as: 
where 𝝈 is the Cauchy stress tensor and 𝝈 the equivalent stress is defined by: 
𝑓 (𝝈, 𝑘) = 𝜎̅̅̅̅̅ − 𝑘 = 0 
𝜎̅̅̅̅̅ = √(𝐏𝝈) ∙ 𝝈 
Where  𝐏  is  a  symmetric  positive-definite  matrix  defined  through  three  independent 
parameters P12, P22, P33: 
𝐏 =
P12
⎡
P12 P22
⎢
⎣
⎤ 
⎥
P33⎦
Flow rule, which defines the incremental plastic strain tensor, is written as follows: 
𝑑𝛆𝑝 = 𝑑𝛿
𝜕𝑔(𝝈)
𝜕𝝈
where  𝑑𝛿  is  a  scalar  plastic  multiplier.    The  plastic  potential  function  𝑔(𝝈)  can  be 
defined as a quadratic function in stress space: 
with, 
𝑔(𝝈) = √(𝐆𝝈) ∙ 𝝈 
𝐆 =
G12
G12 G22
⎡
⎢
⎣
⎤
⎥
G33⎦
When 𝐏𝐆, it leads to non-associated flow rule.  For example, 𝐏 can represent isotropic 
von-Mises  yield  surface  by  setting  P11 = P22 = 1.0,  P12 = −0.5,  P33 = 3.0.    𝐆  can 
represent an orthotropic plastic flow potential by setting: 
𝐺12   =
𝐺22   =
𝐺33   =
, 
𝑟0
1 + 𝑟0
𝑟0(1 + 𝑟90)
𝑟90(1 + 𝑟0)
(1 + 2𝑟45)(𝑟0 + 𝑟90)
𝑟90(1 + 𝑟0)
, 
. 
where  𝑟0, 𝑟45, 𝑟90  are  Lankford  coefficients  in  the  rolling,  diagonal  and  transverse 
direction.    Experiments  have  shown  on  the  stress  level,  some  AHSS,  e.g.,  DP590,  and 
TRIP780 show strong directional dependency of 𝑟-values, while nearly the same stress-
strain  curves  have  been  measured  in  all  directions.    The  directional  dependency  of  𝑟-
values  suggests  planar  anisotropy  while  the  material  response  on  the  stress  level  is 
planar isotropic, which is the main reason to employ the non-associated flow rule. 
On the other hand, if  𝐏 = 𝐆, the associated flow rule is recovered. 
A modified Johnson-Cook plasticity model with mixed Swift-Voce hardening: 
The Johnson-Cook plasticity model (1983) multiplicatively decomposes the deformation 
resistance into three functions representing the effect of strain hardening, strain rate and 
temperature.    The  Johnson-Cook  model  is  modified  to  include  hardening  saturation 
with  a  mixed  Swift-Voce  hardening  law  (Sung  et  al,  A  plastic  constitutive  equation 
incorporating  strain,  strain-rate,  and  temperature,  International  Journal  of  Plasticity,  2010), 
which gives a better description of the hardening at large strain levels, thus improving 
the prediction of the necking and post-necking response of metal sheet: 
𝜎𝑦 = (𝛼(𝐴(𝜀̅𝑝𝑙 + 𝜀0)
) + (1 − 𝛼) (𝑘0 + 𝑄(1 − 𝑒−𝛽𝜀̅𝑝𝑙)))
1 + 𝐶𝑙𝑛
⎜⎜⎜⎛
⎝
 𝜀̇𝑝𝑙
⎟⎞
𝜀0̇ ⎠
⎜⎛
⎝
⎟⎟⎟⎞
⎠
(1
− (
𝑇 − 𝑇𝑟
𝑇𝑚 − 𝑇𝑟
)
) 
where 𝜀̅𝑝𝑙 and 𝜀̇𝑝𝑙 are effective plastic strain and strain rate, respectively; 𝑇𝑚 (TMELT), 𝑇𝑟 
(TREF) and 𝑇 are the melting temperature, reference temperature (ambient temperature
293 kelvin) and current temperature, respectively; 𝑚 (M) is an exponent coefficient.  For 
other symbols’ definitions refer to the aforementioned paper. 
To  make  this  material  model  more  general  and  flexible,  three  load  curves  are  used  to 
define  the  three  components  of  the  deformation  resistance.    A  load  curve  (LCIDS)  is 
used to describe the strain hardening: 
LCIDS:     (𝛼(𝐴(𝜀̅𝑝𝑙 + 𝜀0)
) + (1 − 𝛼) (𝑘0 + 𝑄(1 − 𝑒−𝛽𝜀̅𝑝𝑙))) 
Strain  rate  is  described  by  a  load  curve  LCIDV  (stress  scale  factor  vs.    strain  rates, 
Figure  M260B-1  middle),  which  scales  the  stresses  based  on  the  strain  rates  during  a 
simulation: 
LCIDV:     (1 + 𝐶𝑙𝑛 (
𝑝𝑙
 𝜀̇
𝜀0̇ )) 
The  temperature  softening  effect  is  defined  by  another  load  curve  LCIDT  (stress  scale 
factor vs.  temperature, Figure M260B-1 bottom), which scales the stresses based on the 
temperatures during the simulation: 
LCIDT:     (1 − (
𝑇−𝑇𝑟
𝑇𝑚−𝑇𝑟
)
) 
The  temperature  effect  is  a  self-contained  model,  in  other  words,  it  does  not  require 
thermal exchange with the environment, and it calculates temperatures based on plastic 
strain and strain rate. 
The temperature evolution is determined with: 
𝜂𝑘
𝜌𝐶𝑝
𝑑𝑇 = 𝜔[𝜀̇𝑝𝑙]
𝜎̅̅̅̅̅𝑑𝜀̅𝑝𝑙 
Where 𝜂𝑘 (ETA) is Taylor-Quinney coefficient, 𝜌 (R0) is the mass density and 𝐶𝑝 (CP) is 
the heat capacity; also where, 
𝜔[𝜀̇𝑝𝑙] =
(𝜀̇
⎧
{{{{
{{{{
⎨
⎩
𝑓𝑜𝑟 𝜀̇𝑝𝑙 < 𝜀̇𝑖𝑡
𝑝𝑙−𝜀̇𝑖𝑡)
(3𝜀̇𝑎−2𝜀̇
(𝜀̇𝑎−𝜀̇𝑖𝑡)3
𝑝𝑙−𝜀̇𝑖𝑡)
𝑓𝑜𝑟 𝜀̇𝑖𝑡 ≤   𝜀̇𝑝𝑙 ≤ 𝜀̇𝑎
𝑓𝑜𝑟 𝜀̇𝑎 < 𝜀̇𝑝𝑙
where 𝜀̇𝑖𝑡 > 0 and 𝜀̇𝑎 > 𝜀̇𝑖𝑡 define the limits of the respective domains of isothermal and 
adiabatic conditions (𝜀̇𝑎 = DEPSAD).  For simplification, 𝜀̇𝑖𝑡 = 𝜀̇0(DEPS0).
As  shown  in  a  single  shell  element  uniaxial  stretching  (Figure  M260B-1),  the  general 
effect  of  the  LCIDV  is  to  elevate  the  strain  hardening  behavior  as  the  strain  rate 
increases  (curve  “D”  in  Figure  M260B-2  top),  while  the  effect  of  the  LCIDT  is  strain 
softening as temperature rises (curve “C” in Figure M260B-2 top).  A combined effect of 
both LCIDV and LCIDT may result in strain hardening initially before temperature rise 
enough  to  cause  the  strain  softening  in  the  model  (curve  “E”  in  Figure  M260B-2  top).  
The temperature and strain rates calculated for each element can be viewed with history 
variables #4 and #5 (curves “C” and “D” in Figure M260B-2 bottom), respectively, while 
the  strain  rate  scale  factors  and  temperature  scale  factors  can  be  viewed  with  history 
variable #6 and #7, respectively. 
Rate-dependent Hosford-Coulomb fracture initiation model: 
An  extension  of  the  Hosford-Coulomb  fracture  initiation  model  is  used  to  account  for 
the  effect  of  strain  rate  on  ductile  fracture.    The  damage  accumulation  is  calculated 
through history variable #3, and fracture occurs at an equivalent plastic strain 𝜀̅𝑓  when 
the variable reaches 1.0: 
𝜀𝑓
∫
𝑑𝜀̅𝑝𝑙
𝑝𝑟[𝜂, 𝜃̅]
𝜀̅𝑓
  = 1 
𝑝𝑟,  𝜂, 𝜃̅  are  strain  to  fracture,  stress  triaxiality  and  the  Lode  parameter, 
Where  𝜀̅𝑓
respectively. 
The  fracture  parameters  A,  B0,  GAMMA,  C,  N  (𝑎,   𝑏0,  𝛾,  𝑐,  𝑛)  are  indicated  in  the 
following equations.  Strain to fracture for proportional load: 
𝑝𝑟[𝜂, 𝜃̅] = 𝑏(1 + 𝑐)
𝜀̅𝑓
{
⎜⎜⎜⎜⎜⎛
⎝
((𝑓1 − 𝑓2)𝑎 + (𝑓2 − 𝑓3)𝑎 + (𝑓1 − 𝑓3)𝑎)}
+ 𝑐(2𝜂 + 𝑓1 + 𝑓3)
−1
⎟⎟⎟⎟⎟⎞
⎠
where  𝑎  is  the  Hosford  exponent,  𝑐  is  the  friction  coefficient  controlling  the  effect  of 
triaxiality, 𝑛 is the stress state sensitivity.
The Lode angle parameter dependent trigonometric functions: 
𝑓1[𝜃̅] = 2
3 cos[𝜋
and coefficient 𝑏 (strain to fracture for uniaxial or equi-biaxial stretching): 
6 (3 + 𝜃̅)],      𝑓3[𝜃̅] = − 2
6 (1 − 𝜃̅)],     𝑓2[𝜃̅] = 2
3 cos[𝜋
3 cos[𝜋
6 (1 + 𝜃̅)] 
𝑏 =
{⎧
⎩{⎨
𝑏0
𝑏0 (1 + 𝛾𝑙𝑛 [
𝜀̇𝑝
𝜀̇0
])
𝑓𝑜𝑟 𝜀̇𝑝 < 𝜀̇0 
𝑓𝑜𝑟 𝜀̇𝑝 > 𝜀̇0
where 𝛾 is the strain rate sensitivity. 
Corresponding parameters summary: 
The following table lists variable names used in this material model and corresponding 
symbols employed in the papers: 
P12 
P22 
P33  G12  G22  G33  A 
B0 
GAMMA  C  N 
P12 
P22 
P33  𝐺12  𝐺22  𝐺33 
𝑎 
𝑏0 
𝛾 
𝑐 
𝑛 
TREF  TMELT  M  ETA  CP 
DEPSO  DEPSAD 
R0 
𝑇𝑟 
𝑇𝑚 
𝑚 
𝜂𝑘 
𝐶𝑝 
𝜀̇𝑖𝑡/𝜀̇0 
𝜀̇𝑎 
𝜌 
History variables summary: 
1.  Damage  accumulation:  history  variable  #3.    Elements  will  be  deleted  if  this 
variable  reaches  1.0  for  more  than  half  of  the  through-thickness  integration 
points (Revision 109792). 
2.  Temperatures: history variable #4. 
3.  Strain rates: history variable #5. 
4.  Strain rate scale factors: history variable #6. 
5.  Temperature scale factor: history variable #7.
Keyword example input: 
A  sample  material  input  card  can  be  found  below,  with  parameters  from Mohr,  D.,  et 
al.(2010) and Roth, C.C., Mohr, D. (2014). 
*MAT_MOHR_NON_ASSOCIATED_FLOW 
$#     mid        R0         E        PR       P12       P22       P33       G12 
         1 7.8000E-9   2.10E05  0.300000      -0.5       1.0       3.0   -0.4946 
$      G22       G33     LCIDS     LCIDV     LCIDT      LFLD     LFRAC        W0 
    0.9318    2.4653       100       105       102 
$        A        B0     GAMMA         C         N     SCALE 
      1.97      0.82     0.025      0.00     0.199  3.132E-3 
$     TREF     TMELT         M       ETA        CP      TINI     DEPSO    DEPSAD 
     293.0   1673.70     0.921       0.9     420.0     293.0  0.001164     1.379 
$     AOPT 
         3 
$       XP        YP        ZP        A1        A2        A3 
$       V1        V2        V3        D1        D2        D3      BETA 
       1.0 
*DEFINE_CURVE 
100 
         0.00000E+00         0.30130E+03 
         0.10000E-01         0.42295E+03 
         0.20000E-01         0.47991E+03 
         0.30000E-01         0.52022E+03 
         0.40000E-01         0.55126E+03 
⋮ 
⋮ 
*DEFINE_CURVE 
105 
         0.00000E+00         0.10000E+01 
         0.10000E+00         0.10608E+01 
         0.50000E+00         0.10828E+01 
         0.10000E+01         0.10923E+01 
⋮ 
⋮ 
*DEFINE_CURVE 
102 
         0.29300E+03         0.10000E+01 
         0.33300E+03         0.96168E+00 
         0.37300E+03         0.92744E+00 
         0.41300E+03         0.89459E+00 
         0.45300E+03         0.86261E+00 
⋮ 
⋮ 
Revision information: 
This material model is available in SMP starting in Revision 102375.  Revision history is 
listed below: 
1)  Element deletion feature based on damage accumulation: Revision 109792. 
2)  The option XUE is available starting on Revision 111531.
U n s
i n e d
s h e
Fy
0=
a x i a l
-
U n i
Fy
0=
1.2
1.15
1.1
1.05
1.0
0.0
1.0
0.8
0.6
0.4
0.2
LCIDV
0.5
1.0
Strain rate (x103)
1.5
2.0
LCIDT
0.0
0.4
0.6
0.8
1.0
1.2
1.4
Temperature (x103 kelvin)
Figure  M260B-1.    Uniaxial  stretching  on  a  single  shell  element;  Input  curves
LCIDV and LCIDT.
Pull speed: 15 mm/s, SCALE=1.0
1000
800
600
400
200
)
(
Input
no LCIDV, no LCIDT
no LCIDV, with LCIDT
with LCIDV, no LCIDT
with LCIDV, with LCIDT
0.0
0.2
0.4
0.6
0.8
1.0
Strain
3.0
2.5
2.0
1.5
1.0
0.5
0.0
)
/
(
-
#
Pull speed: 15 mm/s, SCALE=1.0
0.1
0.2
Time (sec)
0.3
500
450
400
350
300
)
(
-
#
250
0.4
Figure M260B-2.  Results of a single element uniaxial stretching - stress-strain
curves (top), strain rates and temperature history under various conditions.
*MAT_LAMINATED_FRACTURE_DAIMLER_PINHO 
This  is  Material  Type  261  which  is  an  orthotropic  continuum  damage  model  for 
laminated fiber-reinforced composites.  See Pinho, Iannucci and Robinson [2006].  It is 
based  on  a  physical  model  for  each  failure  mode  and  considers  non-linear  in-plane 
shear behavior. 
This model is implemented for shell, thick shell and solid elements. 
Remark:  Laminated  shell  theory  can  be  applied  by  setting  LAMSHT ≥  3  in  *CON-
TROL_SHELL. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
EA 
F 
3 
4 
EB 
F 
4 
5 
EC 
F 
5 
6 
7 
8 
PRBA 
PRCA 
PRCB 
F 
6 
F 
7 
F 
8 
Variable 
GAB 
GBC 
GCA 
AOPT 
DAF 
DKF 
DMF 
EFS 
Type 
F 
F 
F 
F 
F 
F 
  Card 3 
Variable 
1 
XP 
Type 
F 
  Card 4 
Variable 
1 
V1 
Type 
F 
2 
YP 
F 
2 
V2 
F 
3 
ZP 
F 
3 
V3 
F 
4 
A1 
F 
4 
D1 
F 
5 
A2 
F 
5 
D2 
F 
F 
7 
F 
8 
7 
8 
6 
A3 
F 
6 
D3 
MANGLE 
F
Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ENKINK 
ENA 
ENB 
ENT 
ENL 
Type 
F 
F 
F 
F 
F 
  Card 6 
Variable 
1 
XC 
Type 
F 
  Card 7 
1 
2 
XT 
F 
2 
3 
YC 
F 
3 
4 
YT 
F 
4 
5 
SL 
F 
5 
6 
7 
8 
Variable 
FIO 
SIGY 
LCSS 
BETA 
PFL 
PUCK 
SOFT 
Type 
F 
F 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
6 
7 
8 
DT 
F 
MID 
RO 
EA 
EB 
EC 
PRBA 
PRCA 
PRCB 
GAB 
GBC 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
𝐸𝑎, Young’s modulus in 𝑎-direction (longitudinal) 
𝐸𝑏, Young’s modulus in 𝑏-direction (transverse) 
𝐸𝑐, Young’s modulus in 𝑐-direction 
𝜈𝑏𝑎, Poisson’s ratio 𝑏𝑎 
𝜈𝑐𝑎, Poisson’s ratio 𝑐𝑎 
𝜈𝑐𝑏, Poisson’s ratio 𝑐𝑏 
𝐺𝑎𝑏, shear modulus 𝑎𝑏 
𝐺𝑏𝑐, shear modulus 𝑏𝑐
GCA 
AOPT 
*MAT_LAMINATED_FRACTURE_DAIMLER_PINHO 
DESCRIPTION
𝐺𝑐𝑎, shear modulus 𝑐𝑎 
Material  axes  option  : 
EQ.0.0:  locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES, and then, for shells only, rotated about
the shell element normal by an angle MANGLE. 
EQ.1.0:  locally orthotropic with material axes determined by a
point  in  space  and  the  global  location  of  the  element
center;  this  is  the  𝑎-direction.    This  option  is  for  solid 
elements only. 
EQ.2.0:  globally orthotropic with material axes determined by 
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0:  locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle (MANGLE) from a line in the plane of the el-
ement defined by the cross product of the vector v with
the element normal. 
EQ.4.0:  locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector  𝐯,  and 
an originating point, 𝐩, which define the centerline ax-
is.  This option is for solid elements only. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
DAF 
Flag  to  control  failure  of  an 
longitudinal (fiber) tensile failure: 
integration  point  based  on
EQ.0.0:  IP fails if any damage variable reaches 1.0. 
EQ.1.0:  no  failure  of  IP  due  to  fiber  tensile  failure.    This
condition  corresponds  to  history  variable  “da(i)” 
reaching 1.0
VARIABLE   
DKF 
DESCRIPTION
Flag  to  control  failure  of  an 
longitudinal (fiber) compressive failure: 
integration  point  based  on
EQ.0.0:  IP fails if any damage variable reaches 1.0. 
EQ.1.0:  no  failure  of  IP  due  to  fiber  compressive  failure.    This
condition  corresponds  to  history  variable  “dkink(i)” 
reaching 1.0. 
DMF 
Flag to control failure of an integration point based on transverse
(matrix) failure: 
EQ.0.0:  IP fails if any damage variable reaches 1.0. 
EQ.1.0:  no  failure  of  IP  due  to  matrix  failure.    This  condition
corresponds to history variable “dmat(i)” reaching 1.0.
EFS 
Maximum  effective  strain  for  element  layer  failure.    A  value  of
unity would equal 100% strain. 
GT.0.0:  fails when effective strain calculated assuming material 
is vol-ume preserving exceeds EFS.  
LT.0.0:  fails  when  effective  strain  calculated  from  the  full
strain tensor exceeds |EFS|. 
XP, YP, ZP 
Coordinates of point p for AOPT = 1 and 4. 
A1, A2, A3 
Define components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
Define components of vector 𝐯 for AOPT = 3. 
D1, D2, D3 
Define components of vector 𝐝 for AOPT = 2. 
MANGLE 
Material  angle  in  degrees  for  AOPT = 0  (shells  only)  and 
AOPT = 3.      MANGLE  may  be  overridden  on  the  element  card,
see *ELEMENT_SHELL_BETA and *ELEMENT_SOLID_ORTHO.
ENKINK 
Fracture  toughness  for  longitudinal  (fiber)  compressive  failure
mode. 
GT.0.0:  The  given  value  will  be  regularized  with 
the
characteristic element length. 
LT.0.0:  Load curve ID = (-ENKINK) which defines the fracture 
toughness for fiber compressive failure mode as a func-
tion of characteristic element length.  No further regu-
larization.
*MAT_LAMINATED_FRACTURE_DAIMLER_PINHO 
DESCRIPTION
ENA 
Fracture toughness for longitudinal (fiber) tensile failure mode. 
GT.0.0:  The  given  value  will  be  regularized  with 
the 
characteristic element length. 
LT.0.0:  Load  curve  ID = (-ENA)  which  defines  the  fracture 
toughness for fiber tensile failure mode as a function of
characteristic  element  length.    No  further  regulariza-
tion. 
ENB 
Fracture toughness for intralaminar matrix tensile failure. 
GT.0.0:  The  given  value  will  be  regularized  with 
the
characteristic element length. 
LT.0.0:  Load  curve  ID = (-ENB)  which  defines  the  fracture 
toughness  for  intralaminar  matrix  tensile  failure  as  a
function  of  characteristic  element  length.    No  further
regularization. 
ENT 
Fracture  toughness  for  intralaminar  matrix  transverse  shear
failure. 
GT.0.0:  The  given  value  will  be  regularized  with 
the
characteristic element length.  
LT.0.0:  Load  curve  ID = (-ENT)  which  defines  the  fracture 
toughness  for  intralaminar  matrix  transverse  shear
failure  as  a  function  of  characteristic  element  length.
No further regularization. 
ENL 
Fracture  toughness  for  intralaminar  matrix  longitudinal  shear
failure. 
GT.0.0:  The  given  value  will  be  regularized  with 
the
characteristic element length.  
LT.0.0:  Load  curve  ID = (-ENL)  which  defines  the  fracture 
toughness  for  intralaminar  matrix  longitudinal  shear 
failure  as  a  function  of  characteristic  element  length.
No further regularization. 
XC 
Longitudinal compressive strength, 𝑎-axis (positive value).  
GT.0.0:  constant value  
LT.0.0:  Load  curve  ID = (-XC)  which  defines  the  longitudinal 
compressive strength vs.  longitudinal strain rate (𝜖 ̇𝑎𝑎).
VARIABLE   
DESCRIPTION
XT 
Longitudinal tensile strength, 𝑎-axis.  
GT.0.0:  constant value  
LT.0.0:  Load  curve  ID = (-XT)  which  defines  the  longitudinal 
tensile strength vs.  longitudinal strain rate (𝜖 ̇𝑎𝑎). 
YC 
Transverse compressive strength, 𝑏-axis (positive value).  
GT.0.0:  constant value  
LT.0.0:  Load  curve  ID = (-YC)  which  defines  the  transverse 
compressive strength vs.  transverse strain rate (𝜖 ̇𝑏𝑏). 
YT 
Transverse tensile strength, 𝑏-axis.  
GT.0.0:  constant value  
LT.0.0:  Load  curve  ID = (-YT)  which  defines  the  transverse 
tensile strength vs.  tansverse strain rate (𝜖 ̇𝑏𝑏). 
SL 
Longitudinal shear strength.  
GT.0.0:  constant value  
LT.0.0:  Load  curve  ID = (-SL)  which  defines  the  longitudinal 
shear strength vs.  in-plane shear strain rate (𝜖 ̇𝑎𝑏). 
FIO 
Fracture  angle  in  pure  transverse  compression  (in  degrees,
default = 53.0). 
SIGY 
In-plane shear yield stress.
*MAT_LAMINATED_FRACTURE_DAIMLER_PINHO 
DESCRIPTION
LCSS 
Load curve ID or Table ID. 
Load Curve.  When LCSS is a Load curve ID, it defines the non-
linear in-plane shear-stress as a function of in-plane shear-strain. 
Tabular Data.  The table maps in-plane strain rate values (𝜖 ̇𝑎𝑏) to 
a  load  curve  giving  the  in-plane  shear-stress  as  a  function  of  in-
plane shear-strain.  For strain rates below the minimum value, the
curve  for  the  lowest  defined  value  of  strain  rate  is  used.
Likewise,  when  the  strain  rate  exceeds  the  maximum  value,  the
curve for the highest defined value of strain rate is used. 
Logarithmically  Defined  Table.    If  the  first  curve  in  the  table 
corresponds to a negative strain rate, LS-DYNA assumes that the 
natural  logarithm  of  the  strain  rate  value  is  used  for  all  stress-
strain curves.  Since the tables are internally discretized to equally
spaced  points,  natural  logarithms  are  necessary,  for  example,  if
the  curves  correspond  to  rates  from  10−4  to  104.    Computing 
natural  logarithms  can  substantially  increase  the  computational 
time on certain computer architectures 
BETA 
Hardening parameter for in-plane shear plasticity (0.0 ≤ BETA ≤
1.0). 
EQ.0.0: 
EQ.1.0: 
Pure kinematic hardening 
Pure isotropic hardening 
0.0 < BETA < 1.0:  mixed hardening. 
PFL 
Percentage  of  layers  which  must  fail  until  crashfront  is  initiated. 
E.g.  |PFL| = 80.0,  then  80%  of  layers  must  fail  until  strengths  are
reduced in neighboring elements.  Default: all layers must fail.  A
single layer fails if 1 in-plane IP fails (PFL > 0) or if 4 in-plane IPs 
fail (PFL < 0). 
PUCK 
Flag  for  evaluation  and  post-processing  of  Puck’s  inter-fiber-
failure criterion (IFF, see Puck, Kopp and Knops [2002]). 
EQ.0.0:  no evaluation of Puck’s IFF-criterion.  
EQ.1.0:  Puck’s IFF-criterion will be evaluated. 
SOFT 
Softening  reduction  factor  for  material  strength  in  crashfront
elements (default = 1.0).
am
−σ
cψ
c ψ
−σ
bψ
−σ
bc
bc
−σ
−σ
cb
cb
−σ
bm
bψ
cψ
−σ
bψ
bψ
ma
c ψ
Matrix fracture plane
−σ
cψ
bψ
mb
mb
Figure M261-1.  Definition of angles and stresses in fracture plane 
  VARIABLE   
DESCRIPTION
DT 
Strain rate averaging option. 
EQ.0.0: Strain rate is evaluated using a running average. 
LT.0.0:  Strain  rate  is  evaluated  using  average  of  last  11  time
steps. 
GT.0.0:  Strain rate is averaged over the last DT time units. 
Remarks: Failure Surfaces 
The  failure  surface  to  limit  the  elastic  domain  is  assembled  by  four  sub-surfaces, 
representing different failure mechanisms.  See Figure M261-1 for definition of angles.  
They are defined as follows: 
1. 
longitudinal (fiber) tension, 
𝑓𝑎 =
𝜎𝑎
𝑋𝑇
= 1  
2. 
longitudinal  (fiber)  compression  (3D-kinking  model)  –  (transformation  to 
fracture plane), 
)
+ (
𝑓𝑘𝑖𝑛𝑘 =
⎧
{{{
⎨
{{{
⎩
(
𝜏𝑇
𝑆𝑇 − 𝜇𝑇𝜎𝑛
𝜎𝑛
𝑌𝑇
)
         (
+ (
𝜏𝑇
𝑆𝑇
𝜏𝐿
𝑆𝐿 − 𝜇𝐿𝜎𝑛
)
+ (
)
)
= 1            𝑖𝑓      𝜎𝑏𝑚 ≤ 0
= 1                 𝑖𝑓      𝜎𝑏𝑚 > 0  
𝜏𝐿
𝑆𝐿
LS-DYNA R10.0
Figure M261-2.  Damage evolution law 
𝑆𝑇 =
𝜎𝑛 =
𝑌𝐶
2 tan(𝜙0)
𝜎𝑏𝑚 + 𝜎𝑐𝜓
   ;     𝜇𝑇 = −
tan(2𝜙0)
   ;     𝜇𝐿 = 𝑆𝐿
𝜇𝑇
𝑆𝑇
+
𝜎𝑏𝑚 − 𝜎𝑐𝜓
cos(2𝜙) + 𝜏𝑏𝑚𝑐𝜓 sin(2𝜙) 
𝜏𝑇 = −
𝜎𝑏𝑚 − 𝜎𝑐𝜓
sin(2𝜙) + 𝜏𝑏𝑚𝑐𝜓 cos(2𝜙) 
𝜏𝐿 = 𝜏𝑎𝑚𝑏𝑚 cos(𝜙) + 𝜏𝑐𝜓𝑎𝑚 sin(𝜙) 
3. 
transverse (matrix) failure: transverse tension,  
𝑓𝑚𝑎𝑡 = (
𝜎𝑛
𝑌𝑇
)
+ (
𝜏𝑇
𝑆𝑇
)
+ (
)
𝜏𝐿
𝑆𝐿
= 1      𝑖𝑓      𝜎𝑛 ≥ 0 
with 
𝜎𝑛 =
+
𝜎𝑏 + 𝜎𝑐
𝜎𝑏 − 𝜎𝑐
𝜎𝑏 − 𝜎𝑐
cos(2𝜙) + 𝜏𝑏𝑐 sin(2𝜙) 
sin(2𝜙) + 𝜏𝑏𝑐 cos(2𝜙) 
𝜏𝑇 = −
𝜏𝐿 = 𝜏𝑎𝑏 cos(𝜙) + 𝜏𝑐𝑎 sin(𝜙) 
4. 
transverse (matrix) failure: transverse compression/shear, 
𝑓𝑚𝑎𝑡 = (
𝜏𝑇
𝑆𝑇 − 𝜇𝑇𝜎𝑛
)
+ (
𝜏𝐿
𝑆𝐿 − 𝜇𝐿𝜎𝑛
)
= 1     𝑖𝑓      𝜎𝑛 < 0 
Remarks: Damange Evolution: 
As  long  as  the  stress  state  is  located  within  the  failure  surface  the  model  behaves 
orthotropic  elastic.    When  reaching  the  failure  criteria  the  effective  (undamaged) 
stresses will be reduced by a factor of (1 − 𝑑), where the damage variable d represents 
failure  mechanisms 
one  of 
the  damage  variables  defined 
the  different 
for
non-linearity defined via
*DEFINE_CURVE
Figure M261-3.  Definition of non-linear in-plane shear behavior 
(𝑑da, 𝑑kink, 𝑑mat).    The  growth  of  these  damage  variables  is  driven  by  a  linear  damage 
evolution  law  based  on  fracture  toughnesses  (𝛤   →  ENKINK,  ENA,  ENB,  ENT,  ENL) 
and  a  characteristic  internal  element  length,  𝐿,  to  account  for  objectivity.    See  Figure 
M261-2. 
Remarks: Nonlinear In-Plane Shear: 
To account for the characteristic non-linear in-plane shear behavior of laminated fiber-
reinforced  composites  a  1D  elasto-plastic  formulation  is  coupled  to  a  linear  damage 
behavior once the maximum allowable stress state for shear failure is reached.  The non-
linearity of the shear behavior can be introduced via the definition of an explicit shear 
stress  vs.    engineering  shear  strain  curve  (LCSS)  with  *DEFINE_CURVE.    See  Figure 
M261-3 (in which epsilon designates engineering shear strain rather than tensorial shear 
strain). 
Remarks: References: 
More  detailed  information  about  this  material  model  can  be  found  in  Pinho,  Iannucci 
and Robinson [2006]. 
Remarks: Element Deletion: 
When  failure  has  occurred  in  all  the  composite  layers  (through-thickness  integration 
points), the element is deleted.  Elements  which  share nodes with the deleted element 
become “crashfront” elements and can have their strengths reduced by using the SOFT 
parameter.    An  earlier  initiation  of  crashfront  elements  is  possible  by  using  the 
parameter PFL.
Remarks: History Variables: 
The number of additional integration point variables written to the LS-DYNA database 
is  input  by  the  *DATABASE_EXTENT_BINARY  definition  with  the  variable  NEIPS 
(shells)  and  NEIPH  (solids).    These  additional  variables  are  tabulated  below  (i  = 
integration point): 
History 
Variable 
Description 
Value 
LS-PrePost 
history variable
fa(i) 
fkink(i) 
fmat(i)  matrix mode 
fiber tensile mode 
fiber compressive mode 
0 → 1:  elastic 
1:  failure criterion rea-
ched 
da(i) 
dkink(i) 
damage fiber tension 
damage 
compression 
fiber 
dmat(i)  damage transverse 
dam(i) 
crashfront 
fmt_p(i) 
fmc_p(i) 
theta_p(i) 
tensile matrix mod 
(Puck criteria) 
compressive 
mode 
(Puck criteria) 
angle of fracture plane 
(radians, Puck criteria) 
matrix 
0:  elastic 
1:  fully damaged 
-1:  element intact 
10 - 8:  element in 
crashfront 
+1:  element failed 
0 → 1:  elastic 
1:  failure criterion rea-
ched 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
11 
12
*MAT_LAMINATED_FRACTURE_DAIMLER_CAMANHO 
This  is  Material  Type  262  which  is  an  orthotropic  continuum  damage  model  for 
laminated  fiber-reinforced  composites.    See  Maimí,  Camanho,  Mayugo  and  Dávila 
[2007].  It is based on a physical model for each failure mode and considers a simplified 
non-linear in-plane shear behavior.  This model is implemented for shell, thick shell and 
solid elements. 
NOTE: Laminated  shell  theory  can  be  applied  by  setting 
LAMSHT ≥ 3 in *CONTROL_SHELL. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
EA 
F 
3 
4 
EB 
F 
4 
5 
EC 
F 
5 
6 
7 
8 
PRBA 
PRCA 
PRCB 
F 
6 
F 
7 
F 
8 
Variable 
GAB 
GBC 
GCA 
AOPT 
DAF 
DKF 
DMF 
EFS 
Type 
F 
F 
F 
F 
F 
F 
  Card 3 
Variable 
1 
XP 
Type 
F 
  Card 4 
Variable 
1 
V1 
Type 
F 
2 
YP 
F 
2 
V2 
F 
3 
ZP 
F 
3 
V3 
F 
4 
A1 
F 
4 
D1 
F 
5 
A2 
F 
5 
D2 
F 
F 
7 
F 
8 
7 
8 
6 
A3 
F 
6 
D3 
MANGLE 
F
Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
GXC 
GXT 
GYC 
GYT 
GSL 
GXCO 
GXTO 
Type 
F 
F 
F 
F 
F 
  Card 6 
Variable 
1 
XC 
Type 
F 
  Card 7 
1 
2 
XT 
F 
2 
3 
YC 
F 
3 
4 
YT 
F 
4 
5 
SL 
F 
5 
F 
6 
F 
7 
XCO 
XTO 
F 
6 
F 
7 
Variable 
FIO 
SIGY 
ETAN 
BETA 
PFL 
PUCK 
SOFT 
Type 
F 
F 
F 
F 
F 
F 
F 
8 
8 
DT 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
EA 
EB 
EC 
PRBA 
PRCA 
PRCB 
GAB 
GBC 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 
𝐸𝑎, Young’s modulus in 𝑎-direction (longitudinal) 
𝐸𝑏, Young’s modulus in 𝑏-direction (transverse) 
𝐸𝑐, Young’s modulus in 𝑐-direction 
𝜈𝑏𝑎, Poisson’s ratio 𝑏𝑎 
𝜈𝑐𝑎, Poisson’s ratio 𝑐𝑎 
𝜈𝑐𝑏, Poisson’s ratio 𝑐𝑏 
𝐺𝑎𝑏, shear modulus 𝑎𝑏 
𝐺𝑏𝑐, shear modulus 𝑏𝑐
VARIABLE   
DESCRIPTION
GCA 
AOPT 
𝐺𝑐𝑎, shear modulus 𝑐𝑎 
Material axes option : 
EQ.0.0:  locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES, and then, for shells only, rotated about 
the shell element normal by an angle MANGLE. 
EQ.1.0:  locally orthotropic with material axes determined by a
point  in  space  and  the  global  location  of  the  element
center;  this  is  the  𝑎-direction.    This  option  is  for  solid 
elements only. 
EQ.2.0:  globally orthotropic with material axes determined by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0:  locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle (MANGLE) from a line in the plane of the el-
ement defined by the cross product of the vector v with
the element normal. 
EQ.4.0:  locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector  𝐯,  and 
an originating point, 𝐩, which define the centerline ax-
is.  This option is for solid elements only. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
DAF 
Flag  to  control  failure  of  an 
longitudinal (fiber) tensile failure: 
integration  point  based  on
EQ.0.0:  IP fails if any damage variable reaches 1.0. 
EQ.1.0:  no failure of IP due to fiber tensile failure, da(i)=1.0
DKF 
*MAT_LAMINATED_FRACTRURE_DAIMLER_CAMANHO 
DESCRIPTION
Flag  to  control  failure  of  an 
longitudinal (fiber) compressive failure: 
integration  point  based  on
EQ.0.0:  IP fails if any damage variable reaches 1.0. 
EQ.1.0:  no  failure  of  IP  due  to  fiber  compressive  failure,
dkink(i) = 1.0. 
DMF 
Flag to control failure of an integration point based on transverse 
(matrix) failure: 
EQ.0.0:  IP fails if any damage variable reaches 1.0. 
EQ.1.0:  no failure of IP due to matrix failure, dmat(i)=1.0 
EFS 
Maximum  effective  strain  for  element  layer  failure.    A  value  of
unity would equal 100% strain. 
GT.0.0:  fails when effective strain calculated assuming material
is vol-ume preserving exceeds EFS.  
LT.0.0:  fails  when  effective  strain  calculated  from  the  full
strain tensor exceeds |EFS|. 
XP YP ZP 
Coordinates of point 𝐩 for AOPT = 1 and 4. 
A1 A2 A3 
Define components of vector 𝐚 for AOPT = 2. 
V1 V2 V3 
Define components of vector 𝐯 for AOPT = 3. 
D1 D2 D3 
Define components of vector 𝐝 for AOPT = 2. 
MANGLE 
Material  angle  in  degrees  for  AOPT = 0  (shells  only)  and 
AOPT = 3.      MANGLE  may  be  overridden  on  the  element  card,
see *ELEMENT_SHELL_BETA and *ELEMENT_SOLID_ORTHO. 
GXC 
Fracture  toughness  for  longitudinal  (fiber)  compressive  failure
mode. 
GT.0.0:  The  given  value  will  be  regularized  with 
the
characteristic element length. 
LT.0.0:  Load  curve  ID = (-GXC)  which  defines  the  fracture 
toughness for fiber compressive failure mode as a func-
tion of characteristic element length.  No further regu-
larization.
VARIABLE   
DESCRIPTION
GXT 
Fracture toughness for longitudinal (fiber) tensile failure mode. 
GT.0.0:  The  given  value  will  be  regularized  with 
the
characteristic element length. 
LT.0.0:  Load  curve  ID = (-GXT)  which  defines  the  fracture 
toughness for fiber tensile failure mode as a function of
characteristic  element  length.    No  further  regulariza-
tion. 
GYC 
Fracture toughness for transverse compressive failure mode. 
GT.0.0:  The  given  value  will  be  regularized  with 
the 
characteristic element length. 
LT.0.0:  Load  curve  ID = (-GYC)  which  defines  the  fracture 
toughness for transverse compressive failure mode as a
function  of  characteristic  element  length.    No  further
regularization. 
GYT 
Fracture toughness for transverse tensile failure mode. 
GT.0.0:  The  given  value  will  be  regularized  with 
the
characteristic element length.  
LT.0.0:  Load  curve  ID = (-GYT)  which  defines  the  fracture 
toughness for transverse tensile failure mode as a func-
tion of characteristic element length.  No further regu-
larization. 
GSL 
Fracture toughness for in-plane shear failure mode. 
GT.0.0:  The  given  value  will  be  regularized  with 
the 
characteristic element length.  
LT.0.0:  Load  curve  ID = (-GSL)  which  defines  the  fracture 
toughness for in-plane shear failure mode as a function 
of characteristic element length.  No further regulariza-
tion.
GXCO 
*MAT_LAMINATED_FRACTRURE_DAIMLER_CAMANHO 
DESCRIPTION
Fracture  toughness  for  longitudinal  (fiber)  compressive  failure
mode to define bi-linear damage evolution. 
GT.0.0:  The  given  value  will  be  regularized  with 
the
characteristic element length.  
LT.0.0:  Load  curve  ID = (-GXCO)  which  defines  the  fracture 
toughness for fiber compressive failure mode to define 
bi-linear damage evolution as a function of characteris-
tic element length.  No further regularization. 
GXTO 
Fracture toughness for longitudinal (fiber) tensile failure mode to
define bi-linear damage evolution. 
GT.0.0:  The  given  value  will  be  regularized  with 
the
characteristic element length.  
LT.0.0:  Load  curve  ID = (-GXTO)  which  defines  the  fracture 
toughness  for  fiber  tensile  failure  mode  to  define  bi-
linear damage evolution as a function of  characteristic
element length.  No further regularization. 
XC 
Longitudinal compressive strength, 𝑎-axis (positive value). 
GT.0.0:  constant value  
LT.0.0:  Load  curve  ID = (-XC)  which  defines  the  longitudinal 
compressive strength vs.  longitudinal strain rate (𝜖 ̇𝑎𝑎). 
XT 
Longitudinal tensile strength, 𝑎-axis. 
GT.0.0:  constant value  
LT.0.0:  Load  curve  ID = (-XT)  which  defines  the  longitudinal 
tensile strength vs.  longitudinal strain rate (𝜖 ̇𝑎𝑎). 
YC 
Transverse compressive strength, 𝑏-axis (positive value).  
GT.0.0:  constant value  
LT.0.0:  Load  curve  ID = (-YC)  which  defines  the  transverse 
compressive strength vs.  transverse strain rate (𝜖 ̇𝑏𝑏). 
YT 
Transverse tensile strength, 𝑏-axis.  
GT.0.0:  constant value  
LT.0.0:  Load  curve  ID = (-YT)  which  defines  the  transverse 
tensile strength vs.  transverse strain rate (𝜖 ̇𝑏𝑏).
VARIABLE   
DESCRIPTION
SL 
Shear strength, 𝑎𝑏 plane.  
GT.0.0:  constant value  
LT.0.0:  Load  curve  ID = (-SL)  which  defines  the  longitudinal 
shear strength vs.  in-plane shear strain rate (𝜖 ̇𝑎𝑏). 
XCO 
Longitudinal  compressive  strength  at  inflection  point  (positive
value).  
GT.0.0:  constant value  
LT.0.0:  Load curve ID = (-XCO) which defines the longitudinal 
compressive strength at inflection point vs.  longitudi-
nal strain rate (𝜖 ̇𝑎𝑎). 
XTO 
Longitudinal tensile strength at inflection point.  
GT.0.0:  constant value  
LT.0.0:  Load curve ID = (-XTO) which defines the longitudinal 
tensile  strength  at  inflection  point  vs.    longitudinal
strain rate (𝜖 ̇𝑎𝑎). 
FIO 
Fracture  angle  in  pure  transverse  compression  (in  degrees, 
default = 53.0). 
SIGY 
In-plane shear yield stress.  
GT.0.0:  constant value  
LT.0.0:  Load  curve  ID = (-SIGY)  which  defines  the  in-plane 
shear yield stress vs.  in-plane shear strain rate (𝜖 ̇𝑎𝑏). 
ETAN 
Tangent modulus for in-plane shear plasticity.  
GT.0.0:  constant value  
LT.0.0:  Load  curve  ID = (-ETAN)  which  defines  the  tangent 
modulus  for  in-plane  shear  plasticity  vs.    in-plane 
shear strain rate (𝜖 ̇𝑎𝑏). 
BETA 
Hardening parameter for in-plane shear plasticity (0.0 ≤ BETA ≤
1.0). 
EQ.0.0: 
EQ.1.0: 
Pure kinematic hardening 
Pure isotropic hardening 
0.0 < BETA < 1.0:  mixed hardening.
PFL 
*MAT_LAMINATED_FRACTRURE_DAIMLER_CAMANHO 
DESCRIPTION
Percentage  of  layers  which  must  fail  until  crashfront  is  initiated.
E.g.  |PFL| = 80.0,  then  80%  of  layers  must  fail  until  strengths  are
reduced in neighboring elements.  Default: all layers must fail.  A
single layer fails if 1 in-plane IP fails (PFL > 0) or if 4 in-plane IPs 
fail (PFL < 0). 
PUCK 
Flag  for  evaluation  and  post-processing  of  Puck’s  inter-fiber-
failure criterion (IFF, see Puck, Kopp and Knops [2002]). 
EQ.0.0:  no evaluation of Puck’s IFF-criterion.  
EQ.1.0:  Puck’s IFF-criterion will be evaluated. 
SOFT 
Softening  reduction  factor  for  material  strength  in  crashfront
elements (default = 1.0). 
DT 
Strain rate averaging option. 
EQ.0.0: Strain rate is evaluated using a running average. 
LT.0.0:  Strain  rate  is  evaluated  using  average  of  last  11  time
steps. 
GT.0.0:  Strain rate is averaged over the last DT time units. 
Remarks: 
The  failure  surface  to  limit  the  elastic  domain  is  assembled  by  four  sub-surfaces, 
representing different failure mechanisms.  They are defined as follows: 
1. 
longitudinal (fiber) tension, 
𝜙1+ =
𝜎11 − 𝜐12𝜎22
𝑋𝑇
= 1  
2. 
longitudinal (fiber) compression – (transformation to fracture plane), 
𝜙1− =
⟨∣𝜎12
𝑚 ∣ + 𝜇𝐿𝜎22
𝑚 ⟩
𝑆𝐿
= 1 
with 
𝜇𝐿 = −
𝑆𝐿 cos(2𝜙0)
𝑌𝐶cos2(𝜙0)
𝜎22
𝑚 = 𝜎11sin2(𝜑𝑐) + 𝜎22cos2(𝜑𝑐) − 2|𝜎12| sin(𝜑𝑐) cos(𝜑𝑐) 
𝑚 = (𝜎22 − 𝜎11) sin(𝜑𝑐) cos(𝜑𝑐) + |𝜎12|(cos2(𝜑𝑐) − sin2(𝜑𝑐)) 
𝜎12
and
𝜑𝑐 = arctan
⎡1 − √1 − 4 (
⎢
⎢
⎢
⎢
⎣
𝑆𝐿
𝑋𝐶
2 (
𝑆𝐿
𝑋𝐶
+ 𝜇𝐿)
𝑆𝐿
𝑋𝐶
+ 𝜇𝐿)
⎤
⎥
⎥
⎥
⎥
⎦
3. 
transverse (matrix) failure: perpendicular to the laminate mid-plane, 
𝜙2+ =
⎧
{
{
{
⎨
{
{
{
⎩
√(1 − 𝑔)
𝜎22
𝑌𝑇
+𝑔 (
𝜎22
𝑌𝑇
)
+ (
)
𝜎12
𝑆𝐿
= 1 𝜎22 ≥ 0
⟨|𝜎12| + 𝜇𝐿𝜎22⟩
𝑆𝐿
= 1
𝜎22 < 0
4. 
transverse (matrix) failure: transverse compression/shear, 
𝜙2− = √(
𝜏𝑇
𝑆𝑇
)
+ (
𝜏𝐿
𝑆𝐿
)
= 1     𝑖𝑓      𝜎22 < 0    
with 
𝜇𝑇 = −
tan(2𝜙0)
𝑆𝑇 = 𝑌𝐶 cos(𝜙0) [sin(𝜙0) +
𝜃 = arctan (
−|𝜎12|
𝜎22 sin(𝜙0)
) 
cos(𝜙0)
tan(2𝜙0)
] 
𝜏𝑇 = ⟨−𝜎22 cos(𝜙0) [sin(𝜙0) − 𝜇𝑇 cos(𝜙0) cos(𝜃)]⟩ 
𝜏𝐿 = ⟨cos(𝜙0) [|𝜎12| + 𝜇𝐿𝜎22 cos(𝜙0) sin(𝜃)]⟩ 
So  long  as  the  stress  state  is  located  within  the  failure  surface  the  model  behaves 
orthotropic  elastic.    The  constitutive  law  is  derived  on  basis  of  a  proper  definition  for 
the ply complementary free energy density 𝐺, whose second derivative with respect to 
the stress tensor leads to the compliance tensor  𝐇 
𝐇 =
𝜕2𝐺
𝜕𝜎 2 =
(1 − 𝑑1)𝐸1
𝜐12
𝐸1
−
−
𝜐21
𝐸2
(1 − 𝑑2)𝐸2
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎣
⎤
⎥
⎥
⎥
⎥
⎥
⎥
(1 − 𝑑6)𝐺12⎦
,
𝑑1 = 𝑑1+
𝑑2 = 𝑑2+
〈𝜎11〉
|𝜎11|
〈𝜎22〉
|𝜎22|
+ 𝑑1−
+ 𝑑2−
〈−𝜎11〉
|𝜎11|
〈−𝜎22〉
|𝜎22|
Damage evolution:
Figure M262-1.  Damage evolution law 
Figure M262-2.  In-plane shear behavior 
Once  the  stress  state  reaches  the  failure  criterion  a  set  of  scalar  damage  variables 
(𝑑1−, 𝑑1+,  𝑑2−, 𝑑2+, 𝑑6) is introduced associated with the different failure mechanisms.  
A bi-linear (longitudinal direction) and a linear (transverse direction) damage evolution 
law is utilized to define the development of the damage variables driven by the fracture 
toughness  and  a  characteristic  internal  element  length  to  account  for  objectivity.    See 
Figure M262-1. 
To account for the characteristic non-linear in-plane shear behavior of laminated fiber-
reinforced composites a 1D elasto-plastic formulation with linear hardening is coupled 
to a linear damage behavior once the maximum allowable stress state for shear failure is 
reached.  See Figure M262-2. 
More detailed information about this material model can be found in Maimí, Camanho, 
Mayugo and Dávila [2007].  
When  failure  has  occurred  in  all  the  composite  layers  (through-thickness  integration 
points), the element is deleted.  Elements  which  share nodes with the deleted element 
become “crashfront” elements and can have their strengths reduced by using the SOFT 
parameter.    An  earlier  initiation  of  crashfront  elements  is  possible  by  using  the 
parameter PFL.  
The number of additional integration point variables written to the LS-DYNA database 
is  input  by  the  *DATABASE_EXTENT_BINARY  definition  with  the  variable  NEIPS
(shells)  and  NEIPH  (solids).    These  additional  variables  are  tabulated  below  (i  = 
integration point): 
Description 
Value 
LS-PrePost 
history variable
History 
Variable 
𝜙1+(i) 
𝜙1−(i) 
𝜙2+(i) 
𝜙2−(i) 
𝑑1+(i) 
𝑑1−(i) 
𝑑2(i) 
𝑑6(i) 
fiber tensile mode 
fiber compressive 
tensile matrix mode 
compressive 
mode 
damage fiber tension 
damage 
compression 
damage transverse 
damage in-plane shear 
matrix 
fiber 
dam(i) 
crashfront 
fmt_p(i) 
fmc_p(i) 
theta_p(i) 
tensile matrix mod 
(Puck criteria) 
compressive 
mode 
(Puck criteria) 
angle of fracture plane 
(radians, Puck criteria) 
matrix 
0 → 1:  elastic 
1:  failure criterion rea-
ched 
0:  elastic 
1:  fully damaged 
-1:  element intact 
10 - 8:  element in 
crashfront 
+1:  element failed 
0 → 1:  elastic 
1:  failure criterion 
reached 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
11 
12
*MAT_TABULATED_JOHNSON_COOK_ORTHO_PLASTICITY 
This  is  Material  Type  264.    This  is  an  orthotropic  elastic  plastic  material  law  with  J3 
dependent yield surface.  This material considers tensile/compressive asymmetry in the 
material  response,  which  is  important  for  HCP  metals  like  Titanium.    The  model  is 
available for solid elements. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
CP 
F 
6 
TR 
F 
7 
8 
BETA 
NUMINT 
F 
F 
Default 
none 
none 
none 
none 
none 
0.0 
1.0 
1.0 
  Card 2 
1 
2 
3 
4 
5 
Variable 
LCT00R 
LCT00T 
LCF 
LCG 
LCH 
Type 
Default 
F 
0 
  Card 3 
1 
F 
0 
2 
F 
0 
3 
F 
0 
4 
Variable 
LCC00R 
LCC00T 
LCS45R 
LCS45T 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
5 
F 
0 
6 
LCI 
F 
0 
6 
7 
8 
7 
8 
SFIEPM 
NITER 
AOPT 
F 
F 
1 
100
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCT90R 
LCT45R 
LCTTHR 
LCC90R 
LCC45R 
LCCTHR 
Type 
Default 
F 
0 
  Card 5 
1 
F 
0 
2 
F 
0 
3 
F 
0 
4 
F 
0 
5 
F 
0 
6 
Variable 
LCT90T 
LCT45T 
LCTTHT 
LCC90T 
LCC45T 
LCCTHT 
F 
0 
2 
YP 
F 
2 
V2 
F 
F 
0 
3 
ZP 
F 
3 
V3 
F 
F 
0 
4 
A1 
F 
4 
D1 
F 
F 
0 
5 
A2 
F 
5 
D2 
F 
F 
0 
6 
A3 
F 
6 
D3 
F 
7 
8 
7 
8 
MACF 
F 
7 
BETA 
F 
8 
Type 
Default 
  Card 6 
Variable 
F 
0 
1 
XP 
Type 
F 
  Card 7 
Variable 
1 
V1 
Type 
F 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density.
*MAT_TABULATED_JOHNSON_COOK_ORTHO_PLASTICITY 
DESCRIPTION
E 
Young’s modulus: 
GT.0.0: constant value is used 
LT.0.0:  temperature  dependent  Young’s  modulus  given  by
load curve ID = -E 
PR 
CP 
TR 
Poisson’s ratio. 
Specific heat. 
Room temperature. 
BETA 
Fraction of plastic work converted into heat. 
NUMINT 
Number of integration points which must fail before the element 
is deleted. 
LCT00R 
LCT00T 
LCF 
LCG 
LCH 
LCI 
EQ.-200: Turns  off  erosion  for  solids.    Not  recommended
unless  used  in  conjunction  with  *CONSTRAINED_-
TIED_NODES_FAILURE. 
Table ID defining for each plastic strain rate value a load curve ID
giving the (isothermal) tensile yield stress versus  plastic strain for 
that rate in the 00 degree direction. 
Table  ID  defining  for  each  temperature  value  a  load  curve  ID
giving  the  (quasi-static)  tensile  yield  stress  versus  plastic  strain
for that temperature in the 00 degree direction. 
Load  curve  ID  or  Table  ID.    The  load  curve  ID  defines  plastic
failure strain as a function of triaxiality.  The table ID defines for
each  Lode  parameter  a  load  curve  ID  giving  the  plastic  failure
strain  versus  triaxiality  for  that  Lode  parameter.    (Table  option 
only for solids and not yet generally supported). 
Load  curve  ID  defining  plastic  failure  strain  as  a  function  of
plastic strain rate. 
Load  curve  ID  defining  plastic  failure  strain  as  a  function  of
temperature 
Load  curve  ID  or  Table  ID.    The  load  curve  ID  defines  plastic
failure  strain  as  a  function  of  element  size.    The  table  ID  defines
for each triaxiality a load curve ID giving the plastic failure strain
versus element size for that triaxiality.
VARIABLE   
LCC00R 
LCC00T 
LCS45R 
LCS45T 
DESCRIPTION
Table ID.  The curves in this table define compressive yield stress
as a function of plastic strain.  The table ID defines for each plastic
strain  rate  value    a  load  curve  ID  giving  the  (isothermal)
compressive yield stress versus plastic strain for that rate in the 00 
direction. 
Table  ID  defining  for  each  temperature  value  a  load  curve  ID
giving the (quasi-static) compressive yield stress versus strain for
that  temperature.    The  curves  in  this  table  define  compressive
yield stress as a function of plastic strain in the 00 direction. 
Table ID.  The load curves define shear yield stress in function of
plastic  strain.    The  table  ID  defines  for  each  plastic  strain  rate
value  a  load  curve  ID  giving  the  (isothermal)  shear  yield  stress
versus plastic strain for that rate in the 45 degree direction. 
Table  ID  defining  for  each  temperature  value  a  load  curve  ID
giving  the  (quasi-static)  shear  yield  stress  versus  strain  for  that
temperature.    The  load  curves  define  shear  yield  stress  as  a
function of plastic strain or effective plastic strain  in 
the 45 degree direction. 
SFIEPM 
Scale factor on the initial estimate of the plastic multiplier. 
NITER 
Maximum number of iterations for the plasticity algorithm
AOPT 
LCT90R 
LCT45R 
LCTTHR 
LCC90R 
LCC45R 
*MAT_TABULATED_JOHNSON_COOK_ORTHO_PLASTICITY 
DESCRIPTION
Material axes option : 
EQ.0.0: locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES,  and  then  rotated  about  the  shell  ele-
ment normal by an angle BETA. 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by 
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0: locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the
element normal. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).    Available  with  the  R3  release 
of Version 971 and later. 
Table ID defining for each plastic strain rate value a load curve ID
giving  the  (isothermal)  tensile  yield    stress  versus    plastic  strain
for that rate in the 90 degree direction. 
Table ID defining for each plastic strain rate value a load curve ID
giving the (isothermal) tensile yield  stress versus plastic strain for
that rate in the 45 degree direction. 
Table ID defining for each plastic strain rate value a load curve ID
giving the (isothermal) tensile yield stress versus plastic strain for
that rate in the thickness degree direction. 
Table ID defining for each plastic strain rate value a load curve ID
giving  the  (isothermal)  compressive  yield    stress  versus    plastic
strain for that rate in the 90 degree direction. 
Table ID defining for each plastic strain rate value a load curve ID
giving  the  (isothermal)  compressive  yield    stress  versus  plastic
strain for that rate in the 45 degree direction.
VARIABLE   
LCCTHR 
LCT90T 
LCT45T 
LCTTHT 
LCC90T 
LCC45T 
LCCTHT 
DESCRIPTION
Table ID defining for each plastic strain rate value a load curve ID
giving  the  (isothermal)  compressive  yield  stress  versus  plastic
strain for that rate in the thickness degree direction. 
Table  ID  defining  for  each  temperature  value  a  load  curve  ID
giving  the  (quasistatic)  tensile  yield    stress  versus    plastic  strain
for that rate in the 90 degree direction. 
Table  ID  defining  for  each  temperature  value  a  load  curve  ID
giving the (quasistatic) tensile yield  stress versus plastic strain for
that rate in the 45 degree direction. 
Table  ID  defining  for  each  temperature  value  a  load  curve  ID
giving the (quasistatic) tensile yield stress versus plastic strain for
that rate in the thickness degree direction. 
Table  ID  defining  for  each  temperature  value  a  load  curve  ID 
giving  the  (quasistatic)  compressive  yield    stress  versus    plastic
strain for that rate in the 90 degree direction. 
Table  ID  defining  for  each  temperature  value  a  load  curve  ID
giving  the  (quasistatic)  compressive  yield    stress  versus  plastic 
strain for that rate in the 45 degree direction. 
Table  ID  defining  for  each  temperature  value  a  load  curve  ID
giving  the  (quasistatic)  compressive  yield  stress  versus  plastic
strain for that rate in the thickness degree direction. 
A1, A2, A3 
Components of vector 𝐚 for AOPT = 2. 
MACF 
Material axes change flag for brick elements: 
EQ.1: No change, default, 
EQ.2: switch material axes 𝑎 and 𝑏, 
EQ.3: switch material axes 𝑎 and 𝑐, 
EQ.4: switch material axes 𝑏 and 𝑐. 
V1, V2, V3 
Components of vector 𝐯 for AOPT = 3. 
D1, D2, D3 
Components of vector 𝐝for AOPT = 2. 
BETA 
Material angle in degrees for AOPT = 0 and 3, may be overridden 
on the element card, see *ELEMENT_SHELL_BETA.
*MAT_TABULATED_JOHNSON_COOK_ORTHO_PLASTICITY 
If IFLAG = 0 the compressive and shear curves are defined as follows: 
σ𝑐(𝜀𝑝𝑐, 𝜀̇𝑝𝑐),     𝜀𝑝𝑐 = 𝜀𝑐 −
σ𝑠(𝛾𝑝𝑠, 𝛾̇𝑝𝑠),     𝛾𝑝𝑠 = 𝛾𝑠 −
𝜎𝑐
𝜎𝑠
,     𝜀̇𝑝𝑐 =  
,     𝛾̇𝑝𝑠 =  
𝜕𝜀𝑝𝑐
𝜕𝑡
𝜕𝛾𝑝𝑠
𝜕𝑡
and two new history variables (#15 plastic strain in compression and #16 plastic strain 
in shear)  are stored in addition to those history variables already stored in MAT_224. 
If IFLAG = 1 the compressive and shear curves are defined as follows: 
σ𝑐(𝜆̇, 𝜆),     𝜎𝑠(𝜆̇, 𝜆),     𝑊𝑝̇ = 𝜎eff𝜆̇ 
History variables may be post-processed through additional variables.  The number of 
additional variables for solids written to the d3plot and d3thdt databases is input by the 
optional  *DATABASE_EXTENT_BINARY  card  as  variable  NEIPH.    The  relevant 
additional variables of this material model are tabulated below:
LS-PrePost  history 
variable # 
5 
6 
7 
8 
9 
10 
11 
12 
13 
14 
15 
16 
Solid elements 
plastic strain rate 
Compressive plastic strain 
Shear plastic strain 
plastic failure strain 
triaxiality 
Lode parameter 
plastic work 
ratio of plastic strain to plastic failure strain 
element size 
temperature 
plastic strain in compression 
plastic strain in shear
*MAT_TISSUE_DISPERSED 
This  is  Material  Type  266.    This  material  is  an  invariant  formulation  for  dispersed 
orthotropy in soft tissues, e.g., heart valves, arterial walls or other tissues where one or 
two collagen fibers are used.  The passive contribution is composed of an isotropic and 
two  anisotropic  parts.    The  isotropic  part  is  a  simple  neo-Hookean  model.    The  first 
anisotropic  part  is  passive,  with  two  collagen  fibers  to  choose  from:  (1)  a  simple 
exponential  model  and  (2)  a  more  advanced  crimped  fiber  model  from  Freed  et  al.  
[2005].  The second anisotropic part is active described in Guccione et al.  [1993] and is 
used for active contraction. 
  Card 1 
1 
Variable 
MID 
Type 
I 
  Card 2 
1 
2 
RO 
F 
2 
Variable 
FID 
ORTH 
Type 
I 
  Card 3 
1 
I 
2 
3 
F 
F 
3 
C1 
F 
3 
4 
5 
6 
7 
8 
SIGMA 
MU 
KAPPA 
ACT 
INIT 
F 
F 
4 
C2 
F 
4 
5 
C3 
F 
5 
F 
6 
I 
7 
THETA 
NHMOD 
F 
6 
F 
7 
I 
8 
8 
Variable 
ACT1 
ACT2 
ACT3 
ACT4 
ACT5 
ACT6 
ACT7 
ACT8 
Type 
F 
  Card 4 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
ACT9 
ACT10 
Type 
F
Card 5 
1 
2 
Variable 
AOPT 
BETA 
Type 
I 
F 
  Card 6 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
XP 
F 
3 
V3 
F 
4 
YP 
F 
4 
D1 
F 
5 
ZP 
F 
5 
D2 
F 
6 
A1 
F 
6 
D3 
F 
7 
A2 
F 
7 
8 
A3 
F 
8 
  VARIABLE   
DESCRIPTION
MID 
Material identification.  A unique number must be specified. 
RO 
F 
SIGMA 
Mass density. 
Fiber dispersion parameter governs the extent to which the  fiber
dispersion extends to the third dimension. F = 0 and F = 1 apply 
to 2D splay with the normal to the membrane being in the  𝛽 and 
the 𝛾-directions, respectively . F = 0.5 applies 
to  3D  splay  with  transverse  isotropy.    Splay  will  be  orthotropic
wheneverF ≠ 0.5. This parameter is ignored if INIT = 1. 
The parameter SIGMA governs the extent of dispersion, such that
as  SIGMA  goes  to  zero,  the  material  symmetry  reduces  to  pure
transverse  isotropy.    Conversely,  as  SIGMA  becomes  large,  the
  This
material  symmetry  becomes  isotropic  in  the  plane. 
parameter is ignored if INIT = 1. 
MU 
MU  is  the  isotropic  shear  modulus  that  models  elastin.    MU
should be chosen such that the following relation is satisfied: 
0.5 (3KAPPA − 2MU) (3KAPPA + MU)
⁄
< 0.5. 
Instability  can  occur  for  implicit  simulations  if  this  quotient  is
close to 0.5.  A modest approach is a quotient between 0.495 and 
0.497. 
KAPPA 
Bulk modulus for the hydrostatic pressure.
ACT 
INIT 
FID 
ORTH 
*MAT_TISSUE_DISPERSED 
DESCRIPTION
ACT = 1  indicates  that  an  active  model  will  be  used  that  acts  in
the  mean  fiber-direction.    The  active  model,  like  the  passive
model, will be dispersed by SIGMA and F, or if INIT = 1, with the 
*INITIAL_FIELD_SOLID keyword. 
INIT = 1  indicates  that  the  anisotropy  eigenvalues  will  be  given
by  *INITIAL_FIELD_SOLID  variables  in  the  global  coordinate 
system . 
The  passive  fiber  model  number.    There  are  two  passive  models 
available: FID = 1 or FID = 2.  They are described in Remark 2. 
ORTH  specifies  the  number  (1  or  2)  of  fibers  used.    When
ORTH = 2 two fiber families are used and arranges symmetrically
THETA  degrees  from  the  mean  fiber  direction  and  lying  in  the 
tissue plane. 
C1-C3 
Passive fiber model parameters. 
THETA 
The angle between the mean fiber direction and the fiber families.
The  parameter  is  active  only  if  ORTH = 2  and  is  particularly 
important in vascular tissues (e.g.  arteries) 
NHMOD 
Neo-Hooke model flag 
ACT1 - 
ACT10 
AOPT 
EQ.0.0: original implementation (modified Neo-Hooke)  
EQ.1.0: standard Neo-Hooke model (as in umat45 of dyn21.f)  
Active fiber model parameters.  Note that ACT10 is an input for a
time  dependent  load  curve  that  overrides  some  of  the  ACTx
values.  See section 2 below. 
Material  axes  option  : 
EQ.0.0:  locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES.  
EQ.2.0:  globally orthotropic with material axes determined by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR.  
EQ.3.0:  locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
2 
𝛽 
3 
𝛾 
𝛼 
Figure M266-1.  The plot  on the left relates  the global coordinates (1, 2, 3) to
the  local  coordinates  (𝛼, 𝛽, 𝛾),  selected  so  the  mean  fiber  direction  in  the
reference  configuration  is  align  with  the  𝛼–axis.    The  plots  on  the  right  show
how  the  unit  vector  for  a  specific  fiber  within  the  fiber  distribution  of  a  3D
tissue is oriented with respect to the mean fiber direction via angles 𝜃 and 𝜙. 
  VARIABLE   
DESCRIPTION
defined  by  the  cross  product  of  the  vector  v  with  the
element normal.  
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available with the R3 release 
of Version 971 and later. 
BETA 
P1 - P3 
Material  angle  in  degrees  for  AOPT = 3,  may  be  overridden  on 
the element card *ELEMANT_SOLID_ORTHO. 
P1, P2 and P3 define the coordinates of point P for AOPT = 1 and 
AOPT = 4. 
A1 - A3 
A1, A2 and A3 define the components of vector A for AOPT = 2. 
D1 - D3 
D1, D2 and D3 define components of vector D for AOPT = 2. 
V1 - V3 
V1, V2 and V3 define  components of vector V for AOPT = 3 and 
AOPT = 4. 
Details  of  the  passive  model  can  be  found  in  Freed  et  al.    (2005)  and  Einstein  et  al.  
(2005).  The stress in the reference configuration consists of a deviatoric matrix term, a 
hydrostatic pressure term, and either one (ORTHO = 1) or two (ORTH = 2) fiber terms:
𝐒 = 𝜅𝐽(𝐽 − 1)𝐂−1 + 𝜇𝐽−2 3⁄ 𝐃𝐄𝐕 [
(𝐈 − 𝐂̅−2)] + 𝐽−2 3⁄ ∑[𝜎𝑖(𝜆𝑖) + 𝜀𝑖(𝜆𝑖)]𝐃𝐄𝐕[𝐊𝑖]
𝑖=1
where S is the second Piola-Kirchhoff stress tensor, J is the Jacobian of the deformation 
gradient, 𝜅 is the bulk modulus, 𝜎𝑖 is the passive fiber stress model used, and 𝜀𝑖 is the 
corresponding active fiber model used.  The operator DEV is the deviatoric projection: 
𝐃𝐄𝐕[•] = (•) −
tr[(•)𝐂]𝐂−1 
where C is the right Cauchy-Green deformation tensor.  The dispersed fourth invariant              
𝜆 = √tr[𝐊𝐂̅], where 𝐂̅is the isochoric part of the Cauchy-Green deformation.  Note that 
𝜆  is  not  a  stretch  in  the  classical  way,  since  K  embeds  the  concept  of  dispersion.  K  is 
called the dispersion tensor or anisotropy tensor and is given in global coordinates.  The 
passive and active fiber models are defined in the fiber coordinate system.  In effect the 
dispersion tensor rotates and weights these one dimensional models, such that they are 
both three-dimensional and in the Cartesian framework. 
In the case where, the splay parameters SIGMA and F are specified, K is given by: 
𝐊𝑖 =
𝐐𝑖
⎡1 + 𝑒−2SIGMA2
⎢⎢⎢
⎣
F(1 − 𝑒−2SIGMA2
) 0
(1 − F)(1 − 𝑒−2SIGMA2
𝑇 
𝐐𝑖
⎤
⎥⎥⎥
)⎦
where Q is the transformation tensor that rotates from the local to the global Cartesian 
system.  In the case when INIT = 1, the dispersion tensor is given by 
𝐊𝑖 = 𝐐𝑖
𝜒𝑖
⎜⎜⎜⎜⎛
⎝
𝜒𝑖
⎟⎟⎟⎟⎞
3⎠
𝜒𝑖
𝑇 
𝐐𝑖
where  the  𝜒:s  are  given  on  the  *INITIAL_FIELD_SOLID  card.    For  the  values  to  be 
3 = 1. It is the responsibility of the user to assure that 
physically meaningful 𝜒𝑖
this condition is met, no internal checking for this is done.  These values typically come 
from diffusion tensor data taken from the myocardium. 
2 + 𝜒𝑖
1 + 𝜒𝑖
Remarks: 
1.  Passive fiber models.  Currently there are two models available. 
a)  If  FID = 1 a crimped fiber model is used.  It is solely developed for colla-
gen fibers.  Given  𝐻0 and 𝑅0 compute:  
𝐿0 = √(2𝜋)2 + (𝐻0)2, Λ =
𝐿0
𝐻0
and
2.5
1.5
0.5
0.98
Crimped Model
Exp Model
1.02
1.04
1.06
1.08
1.1
1.12
1.14
1.16
Stretch
Figure  M266-2.    both  the  Crimped  and  the  Exponential  fiber  models
visualized.  Here  ۓ = 1.1 is the transition point in the crimped model. 
𝐸𝑓 𝐻0
. 
𝐸𝑠 =
𝐻0 + (1 + 37
6𝜋2 + 2
Now if the fiber stretches 𝜆 < Λ the fiber stress is given by: 
𝐿0
𝜋2) (𝐿0 − 𝐻0)
𝜉 =
where 
𝜎 = 𝜉 𝐸𝑠(𝜆 − 1) 
6𝜋2(Λ2 + (4𝜋2 − 1)𝜆2)𝜆
Λ(3𝐻0
2(Λ2 − 𝜆2)(3Λ2 + (8𝜋2 − 3)𝜆2) + 8𝜋2(10Λ2 + (3𝜋2 − 10)𝜆2))
and if 𝜆 > Λ the fiber stress equals: 
𝜎 = 𝐸𝑠(𝜆 − 1) + 𝐸𝑓 (𝜆 − Λ). 
In Figure M266-1 the fiber stress is rendered with 𝐻0 = 27.5, 𝑅0 = 2 and 
the transition point becomes Λ = 1.1. 
b)  The  second  fiber  model  available  (FID = 2)  is  a  simpler  but    more  useful 
model  for  the  general  fiber  reinforced  rubber.    The  fiber  stress  is  simply 
given by: 
𝜎 = 𝐶1 [𝑒
𝐶2
(𝜆2−1)
− 1]. 
The difference between the two fiber models is given in Figure M266-2. 
The  active  model  for  myofibers  (ACT = 1)  is  defined  in  Guccione  et  al.    (1993) 
and is given by:
𝜎 = 𝑇max
where 
𝐶𝑎0
2 + 𝐸𝐶𝑎50
𝐶𝑎0
2 𝐶(𝑡) 
2 =
𝐸𝐶𝑎50
(𝐶𝑎0)max
√𝑒𝐵(𝑙𝑟√2(𝜆−1)+1−𝑙0)−1
and  𝐵  is  a  constant,  (𝐶𝑎0)max  is  the  maximum  peak  intracellular  calcium  con-
centration, 𝑙0 is the sarcomere length at which no active tension develops and 𝑙𝑟 
is the stress free sarcomere length.  The function 𝐶(𝑡) is defined in one of two 
ways.  First it can be given as: 
where  
𝐶(𝑡) =
(1 − cos𝜔(𝑡)) 
𝜔 =
𝑡0
𝑡 − 𝑡0 + 𝑡𝑟
𝑡𝑟
⎧
{
{
{
⎨
{
{
{
⎩
0 ≤ 𝑡 < 𝑡0
𝑡0 ≤ 𝑡 < 𝑡0 + 𝑡𝑟
𝑡0 + 𝑡𝑟 ≤ 𝑡
and 𝑡𝑟 = 𝑚𝑙𝑅𝜆 + 𝑏. Secondly, it can also be given as a load curve.  If a load curve 
should be used its index must be given in ACT10.  Note that all variables that 
correspond to ω are neglected if a load curve is used.  The active parameters on 
Card 3 and 4 are interpreted as: 
ACT1  ACT2 
ACT3 
ACT4 ACT5 ACT6 ACT7 ACT8 ACT9  ACT10
𝑇max  𝐶𝑎0 
(𝐶𝑎0)max 
𝑙0
𝑡0
𝑙𝑅 
LCID 
References: 
1.  Freed  AD.,  Einstein  DR.    and  Vesely  I.,  Invariant  formulation  for  dispersed 
transverse  isotropy  in  aortic  heart  valves  –  An  efficient  means  for  modeling 
fiber splay, Biomechan model Mechanobiol, 4, 100-117, 2005. 
2.  Guccione JM., Waldman LK., McCulloch AD., Mechanics of Active Contraction 
in Cardiac Muscle: Part II – Cylindrical Models of the Systolic Left Ventricle, J.  
Bio Mech, 115, 82-90, 1993.
*MAT_267 
This  is  Material  Type  267.    This  is  an  advanced  rubber-like  model  that  is  tailored  for 
glassy  polymers  and  similar  materials.    It  is  based  on  Arruda´s  eight  chain  model  but 
enhanced with non elastic properties. 
  Card 1 
1 
Variable 
MID 
Type 
I 
2 
RO 
F 
3 
K 
F 
4 
MU 
F 
Default 
none 
none 
0.0 
0.0 
  Card 2 
1 
Variable 
YLD0 
Type 
F 
2 
FP 
F 
3 
GP 
F 
4 
HP 
F 
5 
N 
I 
0 
5 
LP 
F 
6 
7 
8 
MULL 
VISPL 
VISEL 
I 
0 
6 
MP 
F 
I 
0 
7 
NP 
F 
I 
0 
8 
PMU 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 3 
1 
Variable 
M1 
2 
M2 
3 
M3 
4 
M4 
5 
6 
7 
8 
M5 
TIME 
VCON 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
See 
MULL 
See 
MULL 
See 
MULL 
See 
MULL 
See 
MULL 
0.0 
9.0
Variable 
1 
Q1 
Type 
F 
*MAT_EIGHT_CHAIN_RUBBER 
2 
B1 
F 
3 
Q2 
F 
4 
B2 
F 
5 
Q3 
F 
6 
B3 
F 
7 
Q4 
F 
8 
B4 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 5 
Variable 
1 
K1 
Type 
F 
2 
S1 
F 
3 
K2 
F 
4 
S2 
F 
5 
K3 
F 
6 
S3 
F 
7 
8 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 6 
1 
2 
Variable 
AOPT 
MACF 
Type 
F 
F 
3 
XP 
F 
4 
YP 
F 
5 
ZP 
F 
6 
A1 
F 
7 
A2 
F 
8 
A3 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
.0.0 
  Card 7 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
7 
8 
THETA 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0
Card 8-14 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TAUi 
BETAi 
Type 
F 
F 
Default 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
MID 
Material identification.  A unique number must be specified 
RO 
K 
MU 
MULL 
Mass density. 
Bulk modulus.  To get almost incompressible behavior set this to
one  or  two  orders  of  magnitude  higher  than  MU.    Note  that  the
poisons ratio should be kept at a realistic value.  
𝜐 =
3𝐾 − 2𝑀𝑈
2(3𝐾 + 𝑀𝑈)
. 
Shear  modulus.    MU  is  the  product  of  the  number  of  molecular
chains  per  unit  volume  (n),  Boltzmann’s  constant  (k)  and  the
absolute temperature (T).  Thus MU = nkT. 
Parameter  describing  which  softening  algorithm  that  shall  be
used. 
EQ.1: Strain based Mullins effect from Qi and Boyce, see theory 
section below for details 
M1 = A (Qi recommends 3.5) 
M2 = B (Qi recommends 18.0) 
M3 = Z (Qi recommends 0.7) 
M4 = vs (between 0 and 1 and less than vss) 
M5 = vss (between 0 and 1 and greater than vs) 
EQ.2: Energy  based  Mullins,  a  modified  version  of  Roxburgh
and  Ogden  model.    M1 > 0,  M2 > 0  and  M3 > 0  must  be 
set.  See Theory section for details.
VISPL 
*MAT_EIGHT_CHAIN_RUBBER 
DESCRIPTION
Parameter  describing  which  viscoplastic  formulation  that  should
be used, see the theory section for details. 
EQ.0: No viscoplasticity. 
EQ.1: 2 parameters standard model, K1 and S1 must be set. 
EQ.2: 6 parameters G’Sells model, K1,K2,K3,S1,S2 and S3 must
be set. 
EQ.3: 4  parameters  Strain  hardening  model,  K1,K2,S1,S2  must
be set. 
VISEL 
Option for viscoelastic behavior, see the theory section for details.
EQ.0: No viscoelasticity. 
EQ.1: Free energy formulation based on Holzapfel and Ogden.
EQ.2: Formulation based on stiffness ratios from Simo et al. 
YLD0 
Initial yield stress. 
EQ.0.0: No plasticity 
GT.0.0:  Initial yield stress: 
seperataly. 
Hardening 
is 
defined 
LT.0.0:  -YLD0 is taken as the load curve ID for the yield stress
versus effective plastic strain. 
FP-NP 
Parameters  for  Hill’s  general  yield  surface.    For  von  mises  yield
criteria set FP = GP = HP = 0.5 and LP = MP = NP = 1.5. 
PMU 
Kinematic hardening parameter.  It is usually equal to MU. 
M1 - M5 
Mullins parameters 
MULL.EQ.1:  M1 - M5 are used 
MULL.EQ.2:  M1 - M3 are used. 
TIME 
VCON 
A time filter that is used to smoothen out the time derivate of the
strain invariant over a TIME interval.  Default is no smoothening
but a value 100*TIMESTEP is recommended. 
A  material  constant  for  the  volumetric  part  of  the  strain  energy. 
Default  9.0  but  any  value  can  be  used  to  tailor  the  volumetric
response.  For example -2.
VARIABLE   
DESCRIPTION
Q1 - B4 
Voce hardening parameters 
K1 - S3 
Viscoplastic parameters. 
VISPL.EQ.1: K1 and S1 are used. 
VISPL.EQ.2: K1, S1, K2, S2, K3 and S3 are used. 
VISPL.EQ.3: K1, S1 and K2 are used. 
AOPT 
Material  axes  option   for a more complete description. 
EQ.0.0: Locally  orthotropic  with  material  axes  defined  by
element nodes 1, 2 and 4. 
EQ.1.0: Locally orthotropic with material axes determined by a 
point  in  space  and  the  global  location  of  the  element
center; this is the a-direction. 
EQ.2.0: Globally orthotropic with material axes determined by
vectors defined below. 
EQ.3.0: Locally  orthotropic  material  axes  determined  by 
rotating the material axes about the element normal by
and angle THETA.   The angle is defined from the line
in the plane that is defined by the cross product of the
vector v with the element normal.  The plane of a solid
is defined as the midsurface between the inner surface 
and  the  outer  surface defined  by  the  first  4  nodes  and
last 4 nodes. 
EQ.4.0: Locally  orthotropic  in  cylindrical  coordinate  system
with the material axes determined by a vector v and an
originating point P. 
MACF 
Material axes change flag 
EQ.1.0: No change (default) 
EQ.2.0: Switch axes a and b 
EQ.3.0: Switch axes a and c 
EQ.4.0: Switch axes b and c 
XP, YP, ZP 
Define coordinates for point P for AOPT = 1 and 4 
A1, A2, A3 
Define components of vector a for AOPT = 2.
*MAT_EIGHT_CHAIN_RUBBER 
DESCRIPTION
D1, D2, D3 
Define components of vector d for AOPT = 2 
V1, V2, V3 
Define components of vector v for AOPT = 3 and 4 
TAUi 
Relaxation time.  A maximum of 6 values can be used. 
BETAi / 
GAMMAi 
VISEL.EQ.1: Dissipating energy factors. 
VISEL.EQ.2: Gamma factors  
Basic theory: 
This  model  is  based  on  the  work  done  by  Arruda  and  Boyce  [1993],  in  particular 
Arruda’s thesis [1992].  The eight chain rubber model is based on hyper elasticity and it 
is formulated by using strain invariants.  The strain softening is taken from work done 
by   Qi and Boyce [2004], where the strain energy used is defined as 
Ψ = 𝑣𝑠𝜇 [√𝑁Λ𝑐𝛽 + 𝑁ln (
sinh𝛽
)] + Ψ2 = Ψ1 + Ψ2, 
where the amplified chain stretch is given by Λ𝑐 = √𝑋(𝜆̅̅̅̅2 − 1) + 1and  
𝛽 = 𝐿−1
⎜⎛ Λ𝑐
⎟⎞, 
√𝑁⎠
⎝
where 𝜆̅̅̅̅2 = 𝐼1 3⁄ ,  𝜇  is  the  initial  modulus  of  the  soft  domain,  N  is  the  number  of  rigid 
links between crosslinks of the soft domain region. 𝑋 = 1 + 𝐴(1 − 𝑣𝑠) + 𝐵(1 − 𝑣𝑠)2,  is a 
general polynomial describing the interaction between the soft and the hard phases (Qi 
and  Boyce  [2004]  and  Tobin  and  Mullins  [1957]).    The  compressible  behavior  is 
described by the strain energy.  
Ψ2 =
𝜈con
(𝜈conln𝐽 +
𝐽𝜈con
− 1) 
Where J is the determinant of the elastic deformation gradient Fe.  The Cauchy stress is 
then computed as: 
𝝈 =
𝐅𝑒
∂Ψ
∂𝐂𝑒
𝑇 =
𝐅𝑒
𝐅𝑒(𝐒𝟏 + 𝐒𝟐)𝐅𝑒
𝑇 =
𝑣𝑠𝑋𝜇
3𝐽
√𝑁
Λ𝑐
𝐿−1
⎜⎛ Λ𝑐
√𝑁⎠
⎝
⎟⎞ (𝐁𝑒 −
𝐼1𝐈) +
2𝐾
𝐽𝑣con
(1 −
𝐽𝑣con
) 
where 𝐒𝟏 and 𝐒𝟐 are second Piola-Kirchhoff stresses based on Ψ1 and Ψ2 respectively. 
Mullins effect: 
Two models for the Mullins effect are implemented.
1.  MULL = 1 
The strain softening is developed by the evolution law taken from Boyce 2004: 
𝑣̇𝑠 = 𝑍(𝑣𝑠𝑠 − 𝑣𝑠)
√𝑁 − 1
(√𝑁 − Λ𝑐
max)
2 Λ̇ 𝑐
max, 
where  Z  is  a  parameter  that  characterizes  the  evolution  in  𝑣𝑠  with  increasing 
Λ̇ 𝑐
maxis  the 
maximum of Λ𝑐 from the past: 
max.  The  parameter  𝑣𝑠𝑠  is  the  saturation  value  of    𝑣𝑠.  Note  that  Λ̇ 𝑐
Λ̇ 𝑐
max = {
Λ𝑐 < Λ𝑐
Λ̇ 𝑐 Λ𝑐 > Λ𝑐
The  structure  now  evolves  with  the  deformation.    The  dissipation  inequality 
requires  that  the  evolution  of  the  structure  is  irreversible𝑣̇𝑠 ≥ 0.    See  Qi  and 
Boyce [2004]. 
max
max. 
2.  MULL = 3 
The energy driven model based on Ogden and Roxburgh.  When activated the 
strain eergy is automatically transformed to a standard eight chain model.  That 
is, the variables Z, vs and X is automatically set to 0, 1 and 1 respectively.  The 
stress is multiplicative split of the true stress and the softening factor η. 
𝜎̅̅̅̅̅ = 𝜂𝜎,   𝜂 = 1 −
𝑀1
Viscoelasticity: 
1.  VISEL = 1 
erf (
Ψ1
max − Ψ1
𝑀3 − 𝑀2Ψ1
max). 
The viscoelasticity is based on work dine by Holzapfel (2004) 
𝐐̇ 𝛼 +
𝐐𝛼
𝜏𝛼
= 2𝛽𝛼
𝑑𝑡
∂Ψ1
∂𝐂𝑒
= 𝛽𝛼𝐒̇𝟏 
where 𝛼 is the number of viscoelastic terms (0, 1,…, 6). 
2.  VISEL = 2 
With  this  option  the  evolution  is  based  on  work  done  by  Simo  and  Hughes 
(2000). 
𝐐̇ 𝛼 +
𝐐𝛼
𝜏𝛼
= 2
𝛾𝑎
𝜏𝑎
𝑑𝑡
∂Ψ1
∂𝐂𝑒
=
𝛾𝑎
𝜏𝑎
𝐒𝟏 
The the number of Prony terms is restricted to maximum 6 and τ > 0, γ > 0.
The Cauchy stress is obtained by a push forward operation on the total second 
Piola-Kirchhoff stress. 
σ =
𝐅𝑒𝐒𝐅𝑒
𝑇. 
Viscoplasticity: 
The plasticity is based on the general Hills’ yield surface 
2 = 𝐹(𝜎22 − 𝜎33)2 + 𝐺(𝜎33 − 𝜎11)2 + 𝐻(𝜎11 − 𝜎22)2 + 2𝐿𝜎12
𝜎eff
2 + 2𝑀𝜎23
2  
2 + 2𝑁𝜎13
and  the  hardening  is  either  based  on  a  load  curve  ID  (-YLD0)  or  an  extended  Voce 
hardening 
𝜎yld = 𝜎yld0 + 𝑄1(1 − 𝑒𝐵1𝜀̅) + 𝑄2(1 − 𝑒𝐵2𝜀̅) + 𝑄3(1 − 𝑒𝐵3𝜀̅) + 𝑄4(1 − 𝑒𝐵4𝜀̅). 
The yield criterion is written 
𝑓 = 𝜎eff − 𝜎yld ≤ 0. 
Adding  the  viscoplastic  phenomena,  we  simply  add  one  evolution  equation  for  the 
effective plastic strain rate.  Three different formulations is available. 
1.  VISPL = 1 
̇vp = (
𝜀̅
𝑆1
)
. 
𝐾1
where K1 and S1 are viscoplastic material parameters. 
2.  VISPL = 2 
𝜀̇vp =
⎡
⎢⎢
⎣
𝐾3
𝐾1(1 − 𝑒−𝑆1(𝜀vp+𝐾2))𝑒𝑆2𝜀𝑣𝑝
𝑆3
⎤
⎥⎥
⎦
Where K1, K2, K3, S1, S2 and S3 are viscoplastic parameters 
3.  VISPL = 3 
𝜀̇vp = (
𝐾1
𝑆1
)
(𝜀vp + 𝐾2)
𝑆2 
Where K1, K2, S1 and S2 are viscoplastic parameters. 
Kinematic hardening: 
The  back  stress  is  calculated  similar  to  the  Cauchy  stress  above  but  without  the 
softening factors:
β =
𝜇𝑝
3𝐽
√𝑁
Λ𝑐
𝐿−1
⎜⎛ Λ𝑐
√𝑁⎠
⎝
⎟⎞ (𝐈 −
𝐼𝑝𝐂𝑝
−1) 
𝜇𝑝is  a  hardening  material  parameter  (PMU).    The  total  Piola-Kirchhoff  stress  is  now 
given by 𝐒∗ = 𝐒 − β and the total stress is given by a standard push forward operation 
with the elastic deformation gradient. 
Remarks: 
1.  The parameter PMU is usually taken the same as MU. 
2.  For the case of a dilute solution the Mullins parameter A should be equal to 3.5.  
See Qi and Boyce [2004]. 
3.  For a system with well dispersed particles B should somewhere around 18.  See 
Qi and Boyce [2004]. 
References: 
Qi  HJ.,  Boyce  MC.,  Constitutive  model  for  stretch-induced  softening  of  stress-stretch 
behavior  of  elastomeric  materials,  Journal  of  the  Mechanics  and  Physics  of  Solids,  52, 
2187-2205, 2004. 
Arrude EM., Characterization of the strain hardening response of amorphous polymers, 
PhD Thesis, MIT, 1992. 
Mullins  L.,  Tobin  NR.,  Theoretical  model  for  the  elastic  behavior  of  filler  reinforced 
vulcanized rubber, Rubber Chem.  Technol., 30, 555-571, 1957. 
Ogden  RW.    Roxburgh  DG.,  A  pseudo-elastic  model  for  the  Mullins  effect  in  Filled 
rubber., Proc.  R.  Soc.  Lond.  A., 455, 2861-2877, 1999. 
Simo JC., Hughes TJR., Computational Inelasticity, Springer, New York, 2000. 
Holzapfel GA., Nonlinear Solid Mechanics, Wiley, New-York, 2000.
*MAT_BERGSTROM_BOYCE_RUBBER 
This is material type 269.  This is a rubber model based on the Arruda and Boyce (1993) 
chain model accompanied with a viscoelastic contribution according to Bergström and 
Boyce  (1998).    The  viscoelastic  treatment  is  based  on  the  physical  response  of  a  single 
entangled chain in an  embedded polymer gel matrix and the implementation is based 
on Dal and Kaliske (2009).  This model is only available for solid elements. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
K 
F 
4 
G 
F 
5 
GV 
F 
6 
N 
F 
7 
NV 
F 
8 
Default 
none 
none 
none 
none 
none 
none 
none 
  Card 2 
Variable 
Type 
1 
C 
F 
2 
M 
F 
3 
4 
5 
6 
7 
8 
GAM0 
TAUH 
F 
F 
Default 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
MID 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density. 
K 
G 
GV 
N 
Elastic bulk modulus 
Elastic shear modulus 
Viscoelastic shear modulus 
Elastic segment number
VARIABLE   
DESCRIPTION
NV 
Viscoelastic segment number 
C 
M 
Inelastic strain exponent, should be less than zero 
Inelastic stress exponent 
TAUH 
Reference Kirchhoff stress 
Remarks: 
The  deviatoric  Kirchhoff  stress  for  this  model  is  the  sum  of  an  elastic  and  viscoelastic 
part according to 
The elastic part is governed by the Arruda-Boyce strain energy potential resulting in the 
following expression (after a Pade approximation of the Langevin function) 
τ̅̅̅̅̅ = τ𝑒 + τ𝑣 
τ𝑒 =
3 − 𝜆𝑟
1 − 𝜆𝑟
2 (𝐛̅ −
𝑇𝑟(𝐛̅ )
𝐈) 
Here G is the elastic shear modulus, 
is the unimodular left Cauchy-Green tensor, and 
𝐛̅ = 𝐽−2/3𝐅𝐅𝑇 
𝐽 = det 𝐅 
2 =
𝜆𝑟
𝑇𝑟(𝐛̅ )
3𝑁
is the relative network stretch.  
The viscoelastic stress is based on a multiplicative split of the unimodular deformation 
gradient into unimodular elastic and inelastic parts, respectively, 
and we define 
𝐽−1/3𝐅 = 𝐅𝑒𝐅𝑖 
𝑇 
𝐛𝑒 = 𝐅𝑒𝐅𝑒
to be the elastic left Cauchy-Green tensor.  The viscoelastic stress is given as
where 
τ𝑣 =
𝐺𝑣
3 − 𝜆𝑣
2 (𝐛𝑒 −
1 − 𝜆𝑣
𝑇𝑟(𝐛𝑒)
𝐈) 
2 =
𝜆𝑣
𝑇𝑟(𝐛𝑒)
3𝑁𝑣
is the relative network stretch for the viscoelastic part.  The evolution of the elastic left 
Cauchy-Green tensor can be written 
where the inelastic rate-of-deformation tensor is given as 
𝐛̇
𝑒 = 𝐋̅ 𝐛𝑒 + 𝐛𝑒𝐋̅ 𝑇 − 2𝐃𝑖𝐛𝑒 
and  
𝐃𝑖 = 𝛾̇0(𝜆𝑖 − 0.999)𝑐
⎜⎛∥τ𝑣∥
⎟⎞
𝜏̂√2⎠
⎝
𝑚 τ𝑣
∥τ𝑣∥
𝐋̅ = 𝐋 −
𝑇𝑟(𝐋)
𝐈 
is the deviatoric velocity gradient.  The stretch of a single chain relaxing in a polymer is 
linked to the inelastic right Cauchy-Green tensor as 
2 =
𝜆𝑖
𝑇𝐅𝑖)
𝑇𝑟(𝐅𝑖
≥ 1,  
and  this  stretch  is  available  as  the  plastic  strain  variable  in  the  post  processing  of  this 
material.    The  volumetric  part  is  elastic  and  governed  by  the  bulk  modulus,  the 
pressure for this model is given as 
𝑝 = 𝐾(𝐽−1 − 1).
*MAT_270 
This  is  material  type  270.    This  is  a  thermo-elastic-plastic  model  with  kinematic 
hardening  that  allows  for  material  creation  as  well  as  annealing  triggered  by 
temperature.    The  acronym  CWM  stands  for  Computational  Welding  Mechanics, 
Lindström (2013, 2015), and the model is intended to be used for simulating multistage 
weld processes.  This model is available for solid and shell elements. 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
4 
5 
6 
7 
8 
LCEM 
LCPR 
LCSY 
LCHR 
LCAT 
BETA 
Type 
A8 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
None 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TASTART 
TAEND 
TLSTART
TLEND 
EGHOST 
PGHOST  AGHOST 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
Optional Phase Change Card. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
T2PHASE  T1PHASE 
Type 
F 
F 
Default  optional  optional 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified.
RO 
Material density 
LCEM 
Load curve for Young’s modulus as function of temperature 
LCPR 
LCSY 
LCHR 
LCAT 
Load curve for Poisson’s ratio as function of temperature 
Load curve or table for yield stress. 
GT.0:  Yield stress is a load curve as function of temperature. 
LT.0:  |LCSY|  is  a  table  of  yield  curves  for  different  tempera-
tures.  Each yield curve is a function of plastic strain. 
Load  curve  for  hardening  modulus  as  function  of  temperature.
LCHR  is  not  used  for  LCSY.LT.0.    Hardening  modulus  is  then
calculated from yield curve slope.  
Load curve (or table) for thermal expansion coefficient as function
of  temperature  (and  maximum  temperature  up  to  current  time). 
In  the  case  of  a  table,  load  curves  are  listed  according  to  their
maximum temperature.  
BETA 
Fraction isotropic hardening between 0 and 1 
EQ.0:  Kinematic hardening 
EQ.1:  Isotropic hardening 
TASTART 
Annealing temperature start 
TAEND 
Annealing temperature end 
TLSTART 
Birth temperature start 
TLEND 
Birth temperature end 
EGHOST 
Young’s modulus for ghost (quiet) material 
PGHOST 
Poisson’s ratio for ghost (quiet) material 
AGHOST 
Thermal expansion coefficient for ghost (quiet) material 
T2PHASE 
Temperature at which phase change commences 
T1PHASE 
Temperature at which phase change ends
*MAT_270 
This  material is initially in a quiet state, sometimes referred to as a ghost material.  In 
this  state  the  material  has  the  thermo-elastic  properties  defined  by  the  quiet  Young’s 
modulus,  quiet  Poisson’s  ratio  and  quiet  thermal  expansion  coefficient.    These  should 
represent void, i.e., the Young’s modulus should be small enough to not influence the 
surroundings  but  large  enough  to  avoid  numerical  problems.    A  quiet  material  stress 
should  never  reach  the  yield  point.    When  the  temperature  reaches  the  birth 
temperature,  a  history  variable  representing  the  indicator  of  the  welding  material  is 
incremented.  This variable follows 
𝛾(𝑡) = min (1, max [0,
𝑇max − 𝑇𝑙
end − 𝑇𝑙
𝑇𝑙
𝑇(𝑠).  This  parameter  is  available  as  history  variable  9  in the  output 
]) 
start
start
where 𝑇max = max
𝑠≤𝑡
database.  The effective thermo-elastic material properties are interpolated as 
𝐸 = 𝐸(𝑇)𝛾 + 𝐸quiet(1 − 𝛾) 
𝜈 = 𝜈(𝑇)𝛾 + 𝜈quiet(1 − 𝛾) 
𝛼 = 𝛼(𝑇, 𝑇max)𝛾 + 𝛼quiet(1 − 𝛾) 
where  𝐸,  𝜈,  and  𝛼 are  the  Young’s  modulus,  Poisson’s  ratio  and  thermal  expansion 
coefficient, respectively.  Here, the thermal expansion coefficient is either a temperature 
dependent  curve,  or  a  collection  of  temperature  dependent  curves,  ordered  in  a  table 
according  to  maximum  temperature  𝑇max.    The  stress  update  then  follows  a  classical 
isotropic  associative  thermo-elastic-plastic  approach  with  kinematic  hardening  that  is 
summarized  in  the  following.    The  explicit  temperature  dependence  is  sometimes 
dropped for the sake of clarity. 
The stress evolution is given as 
where 𝐂 is the effective elastic constitutive tensor and 
σ̇ = 𝐂(ε̇ − ε̇𝑝 − ε̇𝑇) 
ε̇𝑇 = 𝛼𝑇̇𝐈 
ε̇𝑝 = 𝜀̇𝑝
𝐬 − κ
𝜎̅̅̅̅̅
are the thermal and plastic strain rates, respectively.  The latter expression includes the 
deviatoric stress  
the back stress κ and the effective stress 
𝐬 = 𝛔 −
Tr(𝛔)𝐈, 
𝜎̅̅̅̅̅ = √
(𝐬 − κ): (𝐬 − κ)
that are involved in the plastic equations.  To this end, the effective yield stress is given 
as 
𝜎𝑌 = 𝜎𝑌(𝑇) + 𝛽𝐻(𝑇)𝜀𝑝 
and plastic strains evolve when the effective stress exceeds this value.  The back stress 
evolves as 
κ̇ = (1 − 𝛽)𝐻(𝑇)𝜀̇𝑝
𝐬 − κ
𝜎̅̅̅̅̅
where 𝜀̇𝑝 is the rate of effective plastic strain that follows from consistency equations. 
When  the  temperature  reaches  the  start  annealing  temperature,  the  material  starts 
assuming its virgin properties.  Beyond the start annealing temperature it behaves as an 
ideal  elastic-plastic  material  but  with  no  evolution  of  plastic  strains.    The  resetting  of 
effective plastic properties in the annealing temperature interval is done by modifying 
the effective plastic strain and back stress before the stress update as 
𝑛+1 = 𝜀𝑝
𝜀𝑝
𝑛max [0, min (1,
κ𝑛+1 = κ𝑛max [0, min (1,
𝑇𝑎
end
𝑇 − 𝑇𝑎
start − 𝑇𝑎
end
𝑇 − 𝑇𝑎
start − 𝑇𝑎
𝑇𝑎
)] 
end
)] 
end
The optional Card 3 is used to set history variable 11, which is the average temperature 
rate  by  which  the  temperature  has  gone  from  T2PHASE  to  T1PHASE.    To  fringe  this 
variable  the  range  should  be  set  to  positive  values  since  it  is  during  the  simulation 
temporarily  used  to  store  the  time  when  the  material  has  reached  temperature 
T2PHASE and is then  stored as a negative value.  A strictly positive value means that 
the  material  has  reached  temperature  T2PHASE  and  gone  down  to  T1PHASE  and  the 
history  variable  is  (T2PHASE − T1PHASE) (T1 − T2)
,  where  T2  is  the  time  when 
temperature  T2PHASE  is  reached  and  T1  is  the  time  when  temperature  T1PHASE  is 
reached.  Note that T2PHASE > T1PHASE and T1 > T2.  A value of zero means that the 
element  has  not  yet  reached  temperature  T2PHASE.    A  strictly  negative  value  means 
that the element has reached temperature T2PHASE but not yet T1PHASE. 
⁄
History variable  Description
1-6  Back stress 
7  Temperature at last time step 
8  Yield indicator: 1 if yielding, else 0 
9  Welding material indicator: 0 for ghost material, else 1 
10  Maximum temperature reached 
11  Average temperature rate going from T2PHASE to T1PHASE
*MAT_271 
This is material type 271.  This model is used to analyze the compaction and sintering of 
cemented carbides and the model is based on the works of Brandt (1998).  This material 
is only available for solid elements. 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
4 
5 
6 
7 
8 
P11 
P22 
P33 
P12 
P23 
P13 
Type 
A8 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 2 
Variable 
1 
E0 
2 
LCK 
Type 
F 
F 
3 
PR 
F 
4 
5 
6 
LCX 
LCY 
LCC 
F 
F 
F 
7 
L 
F 
8 
R 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 3 
Variable 
1 
CA 
Type 
F 
2 
CD 
F 
3 
CV 
F 
4 
P 
F 
5 
6 
7 
8 
LCH 
LCFI 
SINT 
TZRO 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
0.0 
none
Sintering Card 1.  Additional card for SINT = 1. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCFK 
LCFS2 
DV1 
DV2 
DS1 
DS2 
OMEGA 
RGAS 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Sintering Card 2.  Additional card for SINT = 1. 
  Card 5 
1 
2 
3 
4 
5 
6 
Variable 
LCPR 
LCFS3 
LCTAU 
ALPHA 
LCFS1 
GAMMA 
Type 
F 
F 
F 
F 
F 
F 
7 
L0 
F 
8 
LCFKS 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
MID 
RO 
PIJ 
E0 
LCK 
PR 
LCX 
LCY 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Initial compactness tensor Pij 
Initial anisotropy variable e (value between 1 and 2) 
Load curve for bulk modulus K as function of relative density d 
Poisson’s ratio   
Load  curve  for  hydrostatic  compressive  yield  X  as  function  of 
relative density d 
Load  curve  for  uniaxial  compressive  yield  Y  as  function  of
relative density d 
LCC 
Load curve for shear yield C0 as function of relative density d
L 
R 
CA 
CD 
CV 
P 
LCH 
LCFI 
Yield surface parameter L relating hydrostatic compressive yield
to point on hydrostatic axis with maximum strength 
Yield  surface  parameter  R  governing  the  shape  of  the  yield
surface 
Hardening parameter ca 
Hardening parameter cd 
Hardening parameter cv 
Hardening exponent p 
Load  curve  giving  back  stress  parameter  H  as  function  of 
hardening parameter e. 
Load  curve  giving  plastic  strain  evolution  angle  ϕ  as  function  of 
relative volumetric stress. 
SINT 
Activate sintering 
EQ.0.0:  Sintering off 
EQ.1.0:  Sintering on 
Absolute zero temperature T0 
Load  curve  fK  for  viscous  compliance  as  function  of  relative
density d 
Load curve fS2 for viscous compliance as function of temperature
T 
Volume diffusion coefficient dV1 
Volume diffusion coefficient dV2 
Surface diffusion coefficient dS1 
Surface diffusion coefficient dS2 
TZRO 
LCFK 
LCFS2 
DV1 
DV2 
DS1 
DS2 
OMEGA 
Blending parameter ω 
RGAS 
LCPR 
Universal gas constant Rgas 
Load  curve  for  viscous  Poisson’s  ratio  ν  as  function  of  relative 
density d
LCFS3 
LCTAU 
ALPHA 
LCFS1 
Load  curve  fS3  for  evolution  of  mobility  factor  as  function  of 
temperature T 
Load curve for relaxation time τ as function of temperature T 
Thermal expansion coefficient α 
Load  curve  fS1  for  sintering  stress  scaling  as  function  of  relative
density d 
GAMMA 
Surface energy density γ affecting sintering stress 
L0 
Grain size l0 affecting sintering stress 
LCFKS 
Load curve fKS scaling bulk modulus as function of temperature
T 
Remarks: 
This model is intended to be used in two stages.  During the first step the compaction of 
a  powder  specimen  is  simulated  after  which  the  results  are  dumped  to  file,  and  in  a 
subsequent  step  the  model  is  restarted  for  simulating  sintering  of  the  compacted 
specimen.    In  the  following,  an  overview  of  the  two  different  models  is  given,  for  a 
detailed description we refer to Brandt (1998).  The progressive stiffening in the material 
during  compaction  makes  it  more  or  less  necessary  to  run  double  precision  and  with 
constraint contacts to avoid instabilities, unfortunately this currently limitates the use of 
this material to the smp version of LS-DYNA. 
The  powder  compaction  model  makes  use  of  a  multiplicative  split  of  the  deformation 
gradient into a plastic and elastic part according to 
𝐅 = 𝐅𝑒𝐅𝑝 
where  the  plastic  deformation  gradient  maps  the  initial  reference  configuration  to  an 
intermediate relaxed configuration 
𝛿𝐱̃ = 𝐅𝑝𝛿𝐗 
and subsequently the elastic part maps this onto the current loaded configuration 
𝛿𝐱 = 𝐅𝑒𝛿𝐱̃ 
The compactness tensor is introduced that maps the intermediate configuration onto a 
virtual fully compacted configuration 
and we define the relative density as 
𝛿𝐱̅ = 𝐏𝛿𝐱̃
𝑑 = det𝐏 =
𝜌̅
where  𝜌  and  𝜌̅  denotes  the  current  and  fully  compacted  density,  respectively.    The 
elastic properties depend highly on the relative density through the bulk modulus 𝐾(𝑑) 
but the Poisson’s ratio is assumed constant. 
Y(d) 
nε
φ(J1/X(d)) 
nε 
C0(d) 
Y(d)
max=(L-
-J1 = σVM 
-X(d)L
-J1 
-
X(d)
The yield surface is represented by two functions in the Rendulic plane according to 
𝜎𝑌(𝑑) =
⎧𝐶0(𝑑) − 𝐶1(𝑑)𝐽1 − 𝐶2(𝑑)𝐽1
{{
√[(𝐿 − 1)𝑋(𝑑)]2 − [𝐽1 − 𝐿𝑋(𝑑)]2
⎨
{{
⎩
𝐽1 ≥ 𝐿𝑋(𝑑)
𝐽1 < 𝐿𝑋(𝑑)
and is in this way capped in both compression and tension, here 
𝐽1 = 3𝜎 𝑚 = 𝑇𝑟(σ). 
The  polynomial  coefficients  in  the  expression  above  are  chosen  to  give  continuity  at 
𝐽1 = 𝐿𝑋(𝑑)  and  to  give  the  uniaxial  compressive  strength  Y(d).  Yielding  is  assumed  to 
occur when the equivalent stress (note the definition) equals the yield stress 
where 
𝜎eq =
𝜎𝑉𝑀
√3
= √
𝐬: 𝐬 ≤ 𝜎𝑌(𝑑) 
𝐬 = σ − 𝜎 𝑚𝐈
⏟⏟⏟⏟⏟
σ𝑑
− κ 
in which the last term is the back stress to be dealt with below.  The yield surface does 
not  depend  on  the  third  stress  invariant.    The  plastic  flow  is  non-assosiated  and  its 
direction is given by 
where  
𝐧𝜀 = (
cos𝜑 −sin𝜑
 sin𝜑   cos𝜑
) 𝐧
∂𝜎𝑌
⎟⎟⎞ 
∂𝐽1
1 ⎠
𝐧 =
𝜎𝑌(𝑑)
⎜⎜⎛
𝜎max ⎝
is the normal to the yield surface as depicted in the Rendulic plane above (note the sign 
of J1).  The angle  φ  is  a function of and defined only for positive values of the relative 
volumetric  stress  J1/X(d)>0,  for  negative  values  φ  is  determined  internally  to  achieve 
smoothness in the plastic flow direction and such that avoid numerical problems at the 
tensile  cap  point.    The  above  equations  are  for  illustrative  purposes,  from  now  on  the 
plastic  flow  direction  is  generalized  to  a  second  order  tensor.    The  plastic  flow  rule  is 
then 
ε̇𝑝 = 𝜆̇𝐧𝜀,
𝑚 =
𝜀̇𝑝
𝑇𝑟(ε̇𝑝),
𝑑 = ε̇𝑝 − 𝜀̇𝑝
ε̇𝑝
𝑚𝐈 
The  evolution  of  the  compactness  tensor  is  directly  related  to  the  evolution  of  plastic 
strain as 
𝐏̇ = −
(ε̇𝑝𝐏 + 𝐏ε̇𝑝) 
and thus the relative density is given by 
𝑑 ̇= −3𝜀̇𝑝
𝑚𝑑 . 
The  back  stress  is  assumed  coaxial  with  the  deviatoric  part  of  the  compactness  tensor 
and given by 
κ = 𝐽1𝐻(𝑒) (𝐏 −
𝑇𝑟(𝐏)
𝐈) 
where e is a measure of intensity of anisotropy.  This takes a value between 1 and 2 and 
evolves with plastic strain and plastic work according to 
𝒆 ̇ = 𝑐𝑎√
where 
𝑑: 𝛆̇𝑝
𝛆̇𝑝
𝑑 − 𝑐𝑣𝐽1𝜀̇𝑝
𝑚𝑊(𝑑, 𝐽1) + 𝑐𝑑𝛆̇𝑝
𝑑: 𝛔𝑊(𝑑, 𝐽1) 
𝑊(𝑑, 𝐽1) = − [
𝐽1
𝑋(𝑑)
]
∫
𝑑0
𝑋(𝜉 )
3𝜉
𝑑𝜉  
and  d0  is  the  density  in  the  initial  uncompressed  configuration.    The  stress  update  is 
completed by the rate equation of stress 
where C(d) is the elastic constitutive matrix. 
𝝈̇ = 𝐂(𝑑): (ε̇ − ε̇𝑝) 
The sintering model is a thermo and viscoelastic model where the evolution of the mean 
and deviatoric stress can be written as
𝜎̇ 𝑚 = 3𝐾𝑠(𝜀̇𝑚 − 𝜀̇𝑇 − 𝜀̇𝑝
𝑚) 
σ̇ 𝑑 = 2𝐺𝑠(ε̇𝑑 − ε̇𝑝
𝑑) 
The thermal strain rate is given by the thermal expansion coefficient as 
𝜀̇𝑇 = 𝛼𝑇̇ 
and  the  bulk  and  shear  modulus  are  the  same  as  for  the  compaction  model  with  the 
exception that they are scaled by a temperature curve 
𝐾𝑠 = 𝑓𝐾𝑆(𝑇)𝐾(𝑑) 
𝐺𝑠 =
3(1 − 2𝜈)
2(1 + 𝜈)
𝐾𝑠 
The inelastic strain rates are different from the compaction model and is here given by 
ε̇𝑝 =
𝝈𝑑
2𝐺𝑣 +
𝜎 𝑚 − 𝜎 𝑠
3𝐾𝑣
𝐈 
which  results  in  a  viscoelastic  behavior  depending  on  the  viscous  compliance  and 
sintering stress.  The viscous bulk compliance can be written 
𝐾𝑣 = 3𝑓𝐾(𝑑) {𝑑𝑉1exp [−
𝑑𝑉2
𝑅𝑔𝑎𝑠(𝑇 − 𝑇0)
] + 𝜔𝑑𝑆1exp [−
𝑑𝑆2
𝑅𝑔𝑎𝑠(𝑇 − 𝑇0)
]} [1 + 𝑓𝑆2(𝑇)𝜉 ] 
from which the viscous shear compliance is modified with aid of the viscous Poisson’s 
ratio 
𝐺𝑣 =
2[1 + 𝜈𝑣(𝑑)]
3[1 − 2𝜈𝑣(𝑑)]
𝐾𝑣 . 
The mobility factor ξ evolves with temperature according to 
and the sintering stress is given as 
𝜉 ̇ =
𝑓𝑆3(𝑇)𝑇̇ − 𝜉
𝜏(𝑇)
𝜎 𝑠 = 𝑓𝑆1(𝑑)
𝑙0
 . 
All this is accompanied with, again, the evolution of relative density given as 
𝑑 ̇= −3𝜀̇𝑝
𝑚𝑑
*MAT_RHT 
This is material type 272.  This model is used to analyze concrete structures subjected to 
impulsive loadings, see Riedel et.al.  (1999) and Riedel (2004). 
  Card 1 
1 
2 
3 
4 
5 
Varriable 
MID 
RO 
SHEAR 
ONEMPA 
EPSF 
Type 
A8 
  Card 2 
Variable 
Type 
1 
A 
F 
  Card 3 
1 
F 
2 
N 
F 
2 
Varriable 
E0C 
E0T 
Type 
F 
  Card 4 
1 
F 
2 
Variable 
GC* 
GT* 
Type 
F 
F 
  Card 5 
1 
Variable 
GAMMA 
Type 
F 
2 
A1 
F 
F 
3 
FC 
F 
3 
EC 
F 
3 
XI 
F 
3 
A2 
F 
6 
B0 
F 
6 
Q0 
F 
6 
7 
B1 
F 
7 
B 
F 
7 
F 
4 
F 
5 
FS* 
FT* 
F 
5 
BETAC 
BETAT 
PTF 
F 
5 
D2 
F 
5 
F 
6 
EPM 
F 
6 
F 
7 
AF 
F 
7 
F 
4 
ET 
F 
4 
D1 
F 
4 
A3 
F 
8 
T1 
F 
8 
T2 
F 
8 
8 
NF 
F 
8 
PEL 
PCO 
NP 
ALPHA0 
F 
F 
F
MID 
RO 
SHEAR 
ONEMPA 
*MAT_272 
DESCRIPTION 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Elastic shear modulus 
Unit conversion factor defining 1 Mpa in the pressure units used.
It  can  also  be  used  for  automatic  generation  of  material
parameters for a given compressive strength.   
EQ.0:  Defaults to 1.0 
EQ.-1:  Parameters generated in m, s and kg (Pa) 
EQ.-2:  Parameters generated in mm, s and tonne (MPa) 
EQ.-3:  Parameters generated in mm, ms and kg (GPa) 
EQ.-4:  Parameters generated in in, s and dozens of slugs (psi) 
EQ.-5:  Parameters generated in mm, ms and g (MPa) 
EQ.-6:  Parameters generated in cm, μs and g (Mbar) 
EQ.-7:  Parameters generated in mm, ms and mg (kPa) 
EPSF 
Eroding plastic strain (default is 2.0) 
B0 
B1 
T1 
A 
N 
FC 
FS* 
FT* 
Q0 
B 
T2 
Parameter for polynomial EOS 
Parameter for polynomial EOS 
Parameter for polynomial EOS 
Failure surface parameter 𝐴 
Failure surface parameter 𝑁 
Compressive strength. 
Relative shear strength 
Relative tensile strength 
Lode angle dependence factor 
Lode angle dependence factor 
Parameter for polynomial EOS
VARIABLE   
DESCRIPTION 
E0C 
E0T 
EC 
ET 
BETAC 
BETAT 
PTF 
GC* 
GT* 
XI 
D1 
D2 
EPM 
AF 
NF 
Reference compressive strain rate 
Reference tensile strain rate 
Break compressive strain rate 
Break tensile strain rate 
Compressive strain rate dependence exponent (optional) 
Tensile strain rate dependence exponent (optional) 
Pressure influence on plastic flow in tension (default is 0.001) 
Compressive yield surface parameter 
Tensile yield surface parameter 
Shear modulus reduction factor 
Damage parameter 
Damage parameter 
Minimum damaged residual strain 
Residual surface parameter 
Residual surface parameter 
GAMMA 
Gruneisen gamma 
A1 
A2 
A3 
PEL 
PCO 
NP 
Hugoniot polynomial coefficient 
Hugoniot polynomial coefficient 
Hugoniot polynomial coefficient 
Crush pressure 
Compaction pressure 
Porosity exponent 
ALPHA 
Initial porosity
*MAT_272 
In  the  RHT  model,  the  shear  and  pressure  part  is  coupled  in  which  the  pressure  is 
described  by  the  Mie-Gruneisen  form  with  a  polynomial  Hugoniot  curve  and  a  p-α 
compaction  relation.    For  the  compaction  model,  we  define  a  history  variable 
representing  the  porosity  𝛼  that  is  initialized  to  𝛼0 > 1.  This  variable  represents  the 
current  fraction  of  density  between  the  matrix  material  and  the  porous  concrete  and 
will decrease with increasing pressure, i.e., the reference density is expressed as 𝛼𝜌.  The 
evolution of this variable is given as 
𝛼(𝑡) = max
⎜⎛1, min
⎝
⎡1 + (𝛼0 − 1) (
⎢
⎣
where 𝑝(𝑡) indicates the pressure at time t.  This expression also involves the initial pore 
crush  pressure  𝑝el,  compaction  pressure  𝑝comp  and  porosity  exponent  𝑁.  For  later  use, 
we define the cap pressure, or current pore crush pressure, as 
𝛼0, min𝑠≤𝑡
⎟⎞ 
⎠
)
𝑝comp − 𝑝(𝑠)
𝑝comp − 𝑝el
}⎫
⎤
⎥
⎭}⎬
⎦
{⎧
⎩{⎨
𝑝𝑐 = 𝑝comp − (𝑝comp − 𝑝el) (
1/𝑁
)
𝛼 − 1
𝛼0 − 1
The  remainder  of  the  pressure  (EOS)  model  is  given  in  terms  of  the  porous  density  𝜌 
and specific internal energy 𝑒 (wrt the porous density).  Depending on user inputs, it is 
either governed by (𝐵0 > 0) 
𝑝(𝜌, 𝑒) =
(𝐵0 + 𝐵1𝜂)𝛼𝜌𝑒 + 𝐴1𝜂 + 𝐴2𝜂2 + 𝐴3𝜂3 𝜂 > 0
{
𝐵0𝛼𝜌𝑒 + 𝑇1𝜂 + 𝑇2𝜂2
𝜂 < 0
or (𝐵0 = 0) 
together with  
𝑝(𝜌, 𝑒) = Γ𝜌𝑒 +
𝑝𝐻(𝜂) = 𝐴1𝜂 + 𝐴2𝜂2 + 𝐴3𝜂3 
𝑝𝐻(𝜂) [1 −
Γ𝜂] 
𝜂(𝜌) =
𝛼𝜌
𝛼0𝜌0
− 1 . 
For the shear strength description we use  
𝑝∗ =
𝑓𝑐
 . 
as the pressure normalized with the compressive strength parameter.  We also use 𝐬 to 
denote  the  deviatoric  stress  tensor  and  𝜀̇𝑝  the  plastic  strain  rate.    The  effective  plastic 
strain is thus denoted ε𝑝 and can be viewed as such in the post processor of choice. 
For a given stress state and rate of loading, the elastic-plastic yield surface for the RHT 
model is given by 
𝜎𝑦(𝑝∗, 𝐬, 𝜀̇𝑝, 𝜀𝑝
∗) = 𝑓𝑐𝜎𝑦
∗(𝑝∗, 𝐹𝑟(𝜀̇𝑝, 𝑝∗), 𝜀𝑝
∗)𝑅3(𝜃, 𝑝∗)
and is the composition of two functions and the compressive strength parameter 𝑓𝑐. The 
first describes the pressure dependence for principal stress conditions 𝜎1 < 𝜎2 = 𝜎3 and 
is expressed in terms of a failure surface and normalized plastic strain as 
𝜎𝑦
∗(𝑝∗, 𝐹𝑟, 𝜀𝑝
∗) = 𝜎𝑓
∗ (
𝑝∗
, 𝐹𝑟) 𝛾 
with 
The failure surface is given as 
𝛾 = 𝜀𝑝
∗ + (1 − 𝜀𝑝
∗)𝐹𝑒𝐹𝑐 . 
∗(𝑝∗, 𝐹𝑟) =
𝜎𝑓
⎡𝑝∗ −
⎢
⎣
𝐹𝑟
+ (
𝐹𝑟
−1
𝑛⁄
)
⎤
⎥
⎦
+ 3𝑝∗ (1 −
∗
𝑓𝑠
𝑄1
)
− 3𝑝∗ (
𝑄2
−
∗
𝑓𝑠
𝑄1𝑓𝑡
∗)
∗
𝐹𝑟𝑓𝑠
𝑄1
∗
𝐹𝑟𝑓𝑠
𝑄1
⎧
{
{
{
{
{
{
{
{
{
{
{
⎨
{
{
{
{
{
{
{
{
{
{
{
⎩
3𝑝∗ ≥ 𝐹𝑟
𝐹𝑟 > 3𝑝∗ ≥ 0
∗
0 > 3𝑝∗ > 3𝑝𝑡
3𝑝𝑡
∗ > 3𝑝∗
∗ =
in  which  𝑝𝑡
factor and 
𝐹𝑟𝑄2𝑓𝑠
∗
∗𝑓𝑡
∗−𝑄2𝑓𝑠
∗)
3(𝑄1𝑓𝑡
  is  the  failure  cut-off  pressure,  𝐹𝑟  is  a  dynamic  increment 
𝑄1 = 𝑅3 (
, 0) 
𝑄2 = 𝑄(𝑝∗) 
∗ are the tensile and shear strength of the concrete relative 
In these expressions, 𝑓𝑡
to the compressive strength 𝑓𝑐 and the Q values are introduced to account for the tensile 
and shear meridian dependence.  Further details are given in the following. 
∗ and 𝑓𝑠
To describe reduced strength on shear and tensile meridian the factor 
𝑅3(𝜃, 𝑝∗) =
2(1 − 𝑄2)cos𝜃 + (2𝑄 − 1)√4(1 − 𝑄2)cos2𝜃 + 5𝑄2 − 4𝑄
4(1 − 𝑄2)cos2𝜃 + (1 − 2𝑄)2
is introduced, where 𝜃 is the Lode angle given by the deviatoric stress tensor s as  
cos3𝜃 =
27 det(𝐬)
2𝜎̅̅̅̅̅(𝐬)3  
𝜎̅̅̅̅̅(𝐬) = √
𝐬: 𝐬 . 
The maximum reduction in strength is given as a function of relative pressure
Finally, the strain rate dependence is given by  
𝑄 = 𝑄(𝑝∗) = 𝑄0 + 𝐵𝑝∗ . 
𝐹𝑟(𝜀̇𝑝, 𝑝∗) =
in which  
𝑐 −
𝐹𝑟
⎧
{
{
⎨
{
{
⎩
𝐹𝑟
3𝑝∗ − 𝐹𝑟
∗ (𝐹𝑟
𝑐 + 𝐹𝑟
𝑡𝑓𝑡
𝐹𝑟
𝐹𝑟
𝑡 − 𝐹𝑟
𝑐) 𝐹𝑟
∗
𝑐 > 3𝑝∗ ≥ −𝐹𝑟
𝑡𝑓𝑡
3𝑝∗ ≥ 𝐹𝑟
𝑡𝑓𝑡
−𝐹𝑟
∗ > 3𝑝∗
𝑡(𝜀̇𝑝) =
𝐹𝑟
⎧
{{{
⎨
{{{
⎩
⎜⎜⎛ 𝜀̇𝑝
𝑡⁄
𝜀̇0
⎝
𝛾𝑐
𝛽𝑐
𝑡⁄
⎟⎟⎞
⎠
√𝜀̇𝑝
𝑡⁄
𝜀̇𝑝
≥ 𝜀̇𝑝
𝑡⁄
𝜀̇𝑝 > 𝜀̇𝑝
 . 
The parameters involved in these expressions are given as (𝑓𝑐 is in MPa below) 
𝛽𝑐 =
𝛽𝑡 =
20 + 3𝑓𝑐
20 + 𝑓𝑐
and 𝛾𝑐/𝑡 is determined from continuity requirements, but it is also possible to choose the 
rate parameters via inputs. 
The elastic strength parameter used above is given by 
𝐹𝑒(𝑝∗) =
⎧
{
{
{
⎨
{
{
{
⎩
∗ −
𝑔𝑐
∗
𝑔𝑐
3𝑝∗ − 𝐹𝑟
∗
𝑐𝑔𝑐
∗𝑓𝑡
∗ + 𝐹𝑟
𝑡𝑔𝑡
𝑐𝑔𝑐
𝐹𝑟
∗
𝑔𝑡
3𝑝∗ ≥ 𝐹𝑟
∗
𝑐𝑔𝑐
∗ (𝑔𝑡
∗ − 𝑔𝑐
∗) 𝐹𝑟
𝑐𝑔𝑐
∗ > 3𝑝∗ ≥ −𝐹𝑟
𝑡𝑔𝑡
∗
∗𝑓𝑡
−𝐹𝑟
𝑡𝑔𝑡
∗𝑓𝑡
∗ > 3𝑝∗
while the cap of the yield surface is represented by 
𝐹𝑐(𝑝∗) =
𝑝∗ ≥ 𝑝𝑐
∗
√1 − (
∗
𝑝∗ − 𝑝𝑢
∗ )
∗ − 𝑝𝑢
𝑝𝑐
∗ > 𝑝∗ ≥ 𝑝𝑢
∗
𝑝𝑐
∗ > 𝑝∗
𝑝𝑢
⎧
{{{
⎨
{{{
⎩
where 
𝑝𝑐
𝑓𝑐
+
∗ =
𝑝𝑐
∗
𝑐𝑔𝑐
𝐹𝑟
𝐺∗𝜀𝑝
𝑓𝑐
∗ =
𝑝𝑢
The hardening behavior is described linearly with respect to the plastic strain, where
, 1
∗ = min
𝜀𝑝
𝜀𝑝
⎟⎞ 
⎜⎛
𝜀𝑝
⎠
⎝
∗)(1 − 𝐹𝑒𝐹𝑐)
𝜎𝑦(𝑝∗, 𝐬, 𝜀̇𝑝, 𝜀𝑝
𝛾3𝐺∗
ℎ =
𝜀𝑝
here 
𝐺∗ = 𝜉𝐺 
where  𝐺  is  the  shear  modulus  of  the  virgin  material  and  𝜉   is  a  reduction  factor 
representing the hardening in the model. 
When hardening states reach the ultimate strength of the concrete on the failure surface, 
damage is accumulated during further inelastic loading controlled by plastic strain.  To 
this end, the plastic strain at failure is given as 
𝑓 =
𝜀𝑝
⎧
{{{{
{{{{
⎨
⎩
𝐷1[𝑝∗ − (1 − 𝐷)𝑝𝑡
∗]𝐷2
𝑝∗ ≥ (1 − 𝐷)𝑝𝑡
∗ + (
𝜀𝑝
(1 − 𝐷)𝑝𝑡
∗ + (
𝜀𝑝
𝐷1
)
⁄
𝐷2
)
𝜀𝑝
𝐷1
⁄
𝐷2
   > 𝑝∗
The damage parameter is accumulated with plastic strain according to 
𝜀𝑝
𝐷 = ∫
𝜀𝑝
𝑑𝜀𝑝
𝜀𝑝
and the resulting damage surface is given as 
𝜎𝑑(𝑝∗, 𝐬, 𝜀̇𝑝) =
⎧
{{{
⎨
{{{
⎩
𝜎𝑦(𝑝∗, 𝐬, 𝜀̇𝑝, 1)(1 − 𝐷) + 𝐷𝑓𝑐𝜎𝑟
∗(𝑝∗)
0 ≤ 𝑝∗
𝜎𝑦(𝑝∗, 𝐬, 𝜀̇𝑝, 1) (1 − 𝐷 −
𝑝∗
∗)
𝑝𝑡
(1 − 𝐷)𝑝𝑡
∗ ≤ 𝑝∗ < 0
where 
∗(𝑝∗) = 𝐴𝑓 {𝑝∗}𝑛𝑓  
𝜎𝑟
Plastic flow occurs in the direction of deviatoric stress, i.e.,  
ε̇𝑝~𝐬 
but for tension there is an option to set the parameter PFC to a number corresponding 
to the influence of plastic volumetric strain.  If 𝜆 ≤ 1 is used to denote this parameter, 
then for the special case of 𝜆 = 1 
ε̇𝑝~𝐬 − 𝑝𝐈
This  was  introduced  to  reduce  noise  in  tension  that  was  observed  on  some  test 
problems.    A  failure  strain  can  be  used  to  erode  elements  with  severe  deformation 
which by default is set to 200%. 
For  simplicity,  automatic  generation  of  material  parameters 
is  available  via 
ONEMPA.LT.0,  then  no  other  parameters  are  needed.    If  FC.EQ.0  then  the  35  MPa 
strength  concrete  in  Riedel  (2004)  is  generated  in  the  units  specified  by  the  value  of 
ONEMPA.  For FC.GT.0 then FC specifies the actual strength of the concrete in the units 
specified  by  the  value  of  ONEMPA.    The  other  parameters  are  generated  by 
interpolating  between  the  35  MPa  and  140  MPa  strength  concretes  as  presented  in 
Riedel (2004).  Any automatically generated parameter may be overridden by the user if 
motivated, one of these parameters may be the initial porosity ALPHA0 of the concrete. 
For post-processing, the following history variables may be of interest 
History variable #2  Internal energy per volume (ρe) 
History variable #3  Porosity value (α) 
History variable #4  Damage value (D) 
or as an alternative use a material history list 
*DEFINE_MATERIAL_HISTORIES Properties 
Label 
Attributes 
Description 
Damage 
- 
- 
- 
-  Damage value 𝐷
*MAT_CONCRETE_DAMAGE_PLASTIC_MODEL 
*MAT_CDPM 
This  is  material  type  273.    CDPM  is  a  damage  plastic  concrete  model  based  on  work 
published  in  Grassl  et  al.    (2011,  2013)  and  Grassl  and  Jirásek  (2006).    This  model  is 
aimed to simulations where failure of concrete structures subjected to dynamic loadings 
is sought.  It describes the characterization of the failure process subjected to multi-axial 
and rate-dependent loading.  The model is based on effective stress plasticity and with a 
damage model based on both plastic and elastic strain measures.  This material model is 
available only for solids. 
There  are  a  lot  of  parameters  for  the  advanced  user  but  note  that  most  of  them  have 
default  values  that  are  based  on  experimental  tests.    They  might  not  be  useful  for  all 
types of concrete and all types of load paths but they are values that can be used as a 
good starting point.  If the default values are not good enough the theory chapter at the 
end of the parameter description can be of use.  
History variables of interest are:  
1 – kappa, 𝜅, see equations below 
15 – damage in tension, 𝜔𝑡, see equations below 
16 – damage in compression, 𝜔𝑐, see equations below 
More details on this material can be found on: 
http://petergrassl.com/Research/DamagePlasticity/CDPMLSDYNA/index.html 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E 
F 
4 
PR 
F 
5 
6 
ECC 
QH0 
F 
F 
7 
FT 
F 
8 
FC 
F 
Default 
none 
none 
none 
0.2 
AUTO 
0.3 
none 
none
Card 2 
Variable 
1 
HP 
Type 
F 
2 
AH 
F 
3 
BH 
F 
4 
CH 
F 
5 
DH 
F 
6 
AS 
F 
7 
DF 
F 
8 
FC0 
F 
Default 
0.5 
0.08 
0.003 
2.0 
1.0E-6 
15.0 
0.85 
AUTO 
  Card 3 
1 
Variable 
TYPE 
Type 
F 
2 
BS 
F 
3 
WF 
4 
5 
6 
7 
8 
WF1 
FT1 
STRFLG 
FAILFLG 
EFC 
F 
F 
F 
F 
F 
F 
Default 
0.0 
1.0 
none  0.15*WF 0.3*FT 
0.0 
0.0 
1.0E-4 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
ECC 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density. 
Young’s  modulus.    The  sign  determines  if  an  anisotropic  (E
positive,  referred  to  as  ISOFLAG = 0  in  the  remarks)  or  an 
isotropic (E negative, referred to as ISOFLAG = 1 in the remarks) 
damage  formulation  is  used.    The  Young’s  modulus  is  taken  as
the absolute value of this parameter. 
Poissons ratio 
Eccentricity parameter. 
EQ.0.0: ECC is calculated from Jirásek and Bazant (2002) as 
ECC =
1 + 𝜖
2 − 𝜖
,
𝜖 =
𝑓𝑡(𝑓𝑏𝑐
𝑓𝑏𝑐(𝑓𝑐
2 − 𝑓𝑐
2 − 𝑓𝑡
2)
2)
,
𝑓𝑏𝑐 = 1.16𝑓𝑐 
QH0 
Initial hardening defined as FC0/FC where FC0 is the compressive 
stress at which the initial yield surface is reached.  Default = 0.3
FT 
FC 
HP 
AH 
BH 
CH 
DH 
AS 
DF 
FC0 
Uniaxial tensile strength (stress) 
Uniaxial compression strength (stress) 
Hardening  parameter.    Default  is  HP = 0.5  which  is  the  value 
used  in  Grassl  et  al.    (2011)  for  strain  rate  dependent  material
response (STRFLG = 1).  For applications without strain rate effect 
(STRFLG = 0)  a  value  of  HP = 0.01  is  recommended,  which  has 
been used in Grassl et al.  (2013). 
Hardening ductility parameter 1 
Hardening ductility parameter 2 
Hardening ductility parameter 3 
Hardening ductility parameter 4 
Ductility parameter during damage 
Flow rule parameter 
Rate  dependent  parameter. 
if  STRFLG = 1. 
Recommended  value  is  10  MPa,  which  has  to  be  entered
consistently with the system of units used. 
  Only  needed 
TYPE 
Flag for damage type. 
EQ.0.0: Linear damage formulation 
EQ.1.0: Bi-linear damage formulation 
EQ.2.0: Exponential damage formulation 
EQ.3.0: No damage 
The best results are obtained with the bi-linear formulation.   
Damage ductility exponent during damage. 
Default = 1.0 
threshold  value 
formulation.
Tensile 
Parameter  controlling  tensile  softening  branch  for  exponential
tensile damage formulation. 
linear  damage 
for 
Tensile  threshold  value  for  the  second  part  of  the  bi-linear 
damage formulation. 
Default = 0.15 × WF 
BS 
WF 
WF1
FT1 
strength 
Tensile 
formulation. 
Default = 0.3 × FT 
STRFLG 
Strain rate flag. 
threshold  value 
for  bi-linear  damage 
EQ.1.0: Strain rate dependent 
EQ.0.0: No strain rate dependency. 
FAILFLG 
Failure flag. 
EQ.0.0: Not active ⇒ No erosion. 
GT.0.0:  Active and element will erode if wt and wc is equal to 
1 in FAIFLG percent of the integration points.  If FAIL-
FLG = 0.60,  60%  of  all  integration  points  must  fail  be-
fore erosion.  
EFC 
Parameter  controlling  compressive  damage  softening  branch  in
the exponential compressive damage formulation. 
Default = 1.0E-4 
Remarks: 
The  stress  for  the  anisotropic  damage  plasticity  model  (E  positive,  ISOFLAG = 0)  is 
defined as 
𝝈 = (1 − 𝜔𝑡)𝝈𝑡 + (1 − 𝜔𝑐)𝝈𝑐 
where 𝝈𝑡 and 𝝈𝑐 are the positive and negative part of the effective stress 𝝈eff determined 
in the principal stress space.  The scalar functions 𝜔𝑡 and 𝜔𝑐 are damage parameters.  
The  stress  for  the  isotropic  damage  plasticity  model  (E  negative,  ISOFLAG = 1)  is 
defined as  
𝝈 = (1 − 𝜔𝑡)𝝈eff
The effective stress 𝝈𝐞𝐟𝐟  is defined according to the damage mechanics convention as  
𝝈𝐞𝐟𝐟 = 𝑫𝒆: (𝜺 − 𝜺𝒑) 
Plasticity: 
The  yield  surface  is  described  by  the  Haigh-Westergaard  coordinates:  the  volumetric 
effective stress 𝜎𝑣, the norm of the deviatoric effective stress 𝜌 and the Lode angle 𝜃, and 
it is given by 
𝑓𝑝(𝜎𝑣, 𝜌, 𝜃, 𝜅) =
[1 − 𝑞1(𝜅)]
⎡
⎢⎢⎢
⎣
− 𝑞1
2(𝜅)𝑞2
2(𝜅) . 
⎜⎜⎛ 𝜌
√6𝑓𝑐
⎝
+
𝜎𝑣
⎟⎟⎞
𝑓𝑐 ⎠
+ √
𝑓𝑐
⎤
⎥⎥⎥
⎦
+ 𝑚0𝑞1(𝜅)2𝑞2(𝜅)
⎡ 𝜌
⎢
√6𝑓𝑐
⎣
𝑟(cos 𝜃) +
𝜎𝑣
⎤
⎥
𝑓𝑐 ⎦
The variables 𝑞1 and 𝑞2 are dependent on the hardening variable 𝜅.  The parameter 𝑓𝑐 is 
the uniaxial compressive strength.  The shape of the deviatoric section is controlled by 
the function 
𝑟(cos 𝜃) =
4(1 − 𝑒2) cos2 𝜃 + (2𝑒 − 1)2
2(1 − 𝑒2) cos 𝜃 + (2𝑒 − 1)√4(1 − 𝑒2) cos2 𝜃 + 5𝑒2 − 4𝑒
where 𝑒 is the eccentricity parameter (ECC).  The parameter 𝑚0 is the friction parameter 
and it is defined as 
𝑚0 =  
where 𝑓𝑡 is the tensile strength. 
3(𝑓𝑐
2 − 𝑓𝑡
𝑓𝑐𝑓𝑡
)
𝑒 + 1
The flow rule is non-associative which means that the direction of the plastic flow is not 
normal to the yield surface.  This is important for concrete since an associative flow rule 
would give an overestimated maximum stress.  The plastic potential is given by 
𝑔(𝜎𝑣, 𝜌, 𝜅) =
{⎧
⎩{⎨
[1 − 𝑞1(𝜅)]
⎜⎛ 𝜌
√6𝑓𝑐
⎝
+
𝜎𝑣
⎟⎞
𝑓𝑐 ⎠
+ √
}⎫
𝑓𝑐⎭}⎬
+ 𝑞1(𝜅)
⎜⎛𝑚0𝜌
√6𝑓𝑐
⎝
+
𝑚𝑔(𝜎𝑣, 𝜅)
𝑓𝑐
⎟⎞ 
⎠
where  
and 
𝑚𝑔(𝜎𝑣, 𝜅) = 𝐴𝑔(𝜅)𝐵𝑔(𝜅)𝑓𝑐𝑒
𝜎𝑣−𝑞2𝑓𝑡/3
𝐵𝑔𝑓𝑐
𝐴𝑔 =
3𝑓𝑡𝑞2(𝜅)
𝑓𝑐
+
𝑚0
,
𝐵𝑔 =
𝑞2(𝜅)
1 + 𝑓𝑡/𝑓𝑐
ln
𝐴𝑔
3𝑞2 +
𝑚0
  + ln (
𝐷𝑓 + 1
2𝐷𝑓 − 1
)
The  hardening  laws  𝑞1  and  𝑞2  control  the  shape  of  the  yield  surface  and  the  plastic 
potential, and they are defined as 
𝑞1(𝜅) = 𝑞ℎ0 + (1 − 𝑞ℎ0)(𝜅3 − 3𝜅2 + 3𝜅) − 𝐻𝑝(𝜅3 − 3𝜅2 + 2𝜅),
𝜅 < 1 
𝑞1(𝜅) = 1,                                                                                                              𝜅 ≥ 1 
𝑞2(𝜅) = 1,                                                                                                              𝜅 < 1 
𝑞2(𝜅) = 1 + 𝐻𝑝(𝜅 − 1),                                                                                     𝜅 ≥ 1 
The evolution for the hardening variable is given by 
4𝜆̇ cos2 𝜃
𝑥ℎ(𝜎𝑣)
It sets the rate of the hardening variable to the norm of the plastic strain rate scaled by a 
ductility measure which is defined below as 
𝑑𝑔
𝑑𝜎
𝜅̇ =
∥ 
∥
−
𝑥ℎ(𝜎𝑣) = 𝐴ℎ − (𝐴ℎ − 𝐵ℎ)𝑒
𝑅ℎ
𝐹ℎ + 𝐷ℎ,                      𝑅ℎ < 0   
𝑅ℎ
𝐶ℎ,      𝑅ℎ ≥ 0 
𝑥ℎ(𝜎𝑣) = 𝐸ℎ𝑒
And finally 
Damage: 
𝐸ℎ = 𝐵ℎ − 𝐷ℎ,
𝐹ℎ =
(𝐵ℎ − 𝐷ℎ)𝐶ℎ
𝐴ℎ − 𝐵ℎ
Damage is initialized when the equivalent strain 𝜀̃ reaches the threshold value 𝜀0 = 𝑓𝑡 𝐸⁄  
where the equivalent strain is defined as 
𝜀̃ =
𝜀0𝑚0
⎡ 𝜌
⎢
2 ⎣
√6𝑓𝑐
𝑟(𝑐𝑜𝑠𝜃) +
𝜎𝑉
⎤ +
⎥
𝑓𝑐 ⎦
2𝑚0
𝜀0
4 ⎝
⎜⎛ 𝜌
√6𝑓𝑐
𝑟(𝑐𝑜𝑠𝜃) +
𝜎𝑉
⎟⎞
𝑓𝑐 ⎠
+
2𝜌2
3𝜀0
2  
2𝑓𝑐
√
√√
⎷
Tensile  damage  is  described  by  a  stress-inelastic  displacement  law.    For  linear  and 
exponential  damage  type  the  stress  value  𝑓𝑡  and  the  displacement  value  𝑤𝑓   must  be 
defined.  For the bi-linear type two additional parameters 𝑓𝑡1 and 𝑤𝑓1 must be defined, 
see figure below how the stress softening is controlled by the input parameters.
𝜎𝑡 
𝑓𝑡 
𝜎𝑡
𝑓𝑡 
𝑓𝑡1 
𝜎𝑡
𝑓𝑡
𝑤𝑓  
𝜀𝑡ℎ 
𝑤𝑓1
𝑤𝑓
𝜀𝑡ℎ
𝑤𝑓  
𝜀𝑡ℎ
The variable ℎ is a mesh-dependent measure used to convert strains to displacements.  
The  variable    𝜀𝑡  is  called  the  inelastic  tensile  strain  and  is  defined  as  the  sum  of  the 
irreversible  plastic  strain  𝜀𝑝  and  the  reversible  strain  𝑤𝑡(𝜀 − 𝜀𝑝)  (in  compression 
𝑤𝑐(𝜀 − 𝜀𝑝)).  To get the influence of multi-axial stress states on the softening a damage 
ductility measure 𝑥𝑠 is added: 
Where 𝐴𝑠 and 𝐵𝑠 are input parameters, and 
𝑥𝑠 = 1 + (𝐴𝑠 − 1)𝑅𝑠
𝐵𝑠 
𝑅𝑠 = −
√6𝜎𝑣
,
𝜎𝑣 < 0  𝑎𝑛𝑑  𝑅𝑠 = 0,
𝜎𝑣 > 0  
The inelastic strain is then modified according: 
𝜀𝑖
𝑥𝑠
𝜀𝑖 =
Compressive damage is controlled by an exponential stress-inelastic strain law.  Stress 
value  𝒇𝒄  and  inelastic  strain  𝜺𝒇𝒄  need  to  be  specified,  see  figure  below  how  the  stress 
softening  is  controlled  by  the  input  parameters.    A  small  value  of  𝜺𝒇𝒄,  i.e.    1.0E-4 
(default),  provides for a rather brittle form of damage. 
𝜎𝑐 
𝑓𝑐 
𝐴𝑠 𝜀𝑓𝑐 
𝜀𝑐
Strain rate: 
Concrete  is  strongly  rate  dependent.    If  the  loading  rate  is  increased,  the  tensile  and 
compressive strength increase and are more prominent in tension then in compression.  
The  dependency  is  taken  into  account  by  an  additional  variable  𝛼𝑟 ≥ 1.  The  rate 
dependency  is  included  by  scaling  both  the  equivalent  strain  rate  and  the  inelastic 
strain.  The rate parameter is defined by 
𝛼𝑟 = (1 − 𝑋compression) 𝛼𝑟𝑡 + 𝑋compression𝛼𝑟𝑐 
Where 𝑋compression is continuous compression measure (= 1 means only compression, = 0 
means only tension) and for tension we have 
𝛼𝑟𝑡 =
𝛿𝑡
⎧
)
(
{{{{{
{{{{{
𝛽𝑡 (
⎩
𝜀̇max
𝜀̇𝑡0
𝜀̇max
𝜀̇𝑡0
⎨
𝜀̇max < 30 × 10−6𝑠−1 
30 × 10−6 < 𝜀̇max < 1 𝑠−1
)
 𝜀̇max > 1 𝑠−1
where 𝛿𝑡 = 1
rate factor is given by 
1+8𝑓𝑐/𝑓𝑐0
 , 𝛽𝑡 = 𝑒6𝛿𝑡−2 and 𝜀̇𝑡0 = 1 × 10−6𝑠−1. For compression the corresponding 
𝛼𝑟𝑐 =
⎧1
[𝑆
{{{{{
{{{{{
𝛽𝑐 [
⎩
⎨
]
|𝜀̇min|
𝜀̇𝑐0
|𝜀̇min|
𝜀̇𝑐0
1.026𝛿𝑐
|𝜀̇min| < 30 × 10−6𝑠−1
30 × 10−6 < |𝜀̇min| < 1𝑠−1
]
| 𝜀̇min| > 30𝑠−1
where  𝛿𝑐 = 1
parameter.  A recommended value is 10MPa.
5+9𝑓𝑐/𝑓𝑐0
,  𝛽𝑐 = 𝑒6.156𝛿𝑐−2  and  𝜀̇𝑐0 = 30 × 10−6𝑠−1.  The  parameter  𝑓𝑐0  is  an  input
*MAT_PAPER 
This is material type 274.  This is an orthotropic elastoplastic model for paper materials, 
based  on  Xia  (2002)  and  Nygards  (2009),  and  is  available  for  solid  and  shell  elements.  
Solid  elements  use  a  hyperelastic-plastic  formulation,  while  shell  elements  use  a 
hypoelastic-plastic formulation. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
E1 
F 
4 
E2 
F 
5 
E3 
F 
6 
7 
8 
PR21 
PR32 
PR31 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
Variable 
G12 
G23 
G13 
E3C 
Type 
F 
F 
F 
F 
5 
CC 
F 
TWOK 
F 
6 
7 
8 
Default 
none 
none 
none 
none 
none 
none 
ROT 
F 
0.0 
In plane Yield Surface Card 1. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
S01 
A01 
B01 
C01 
S02 
A02 
B02 
C02 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none
*MAT_274 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
S03 
A03 
B03 
C03 
S04 
A04 
B04 
C04 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
In plane Yield Surface Card 3. 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
S05 
A05 
B05 
C05 
PRP1 
PRP2 
PRP4 
PRP5 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
1/2 
2/15 
1/2 
2/15 
Out of Plane and Transverse Shear Yield Surface Card. 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ASIG 
BSIG 
CSIG 
TAU0 
ATAU 
BTAU 
Type 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none
Card 7 
1 
2 
Variable 
AOPT 
MACF 
Type 
F 
F 
*MAT_PAPER 
3 
XP 
F 
4 
YP 
F 
5 
ZP 
F 
6 
A1 
F 
7 
A2 
F 
8 
A3 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Orthotropic Parameter Card 2. 
  Card 8 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
7 
8 
BETA 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
MID 
RO 
Ei 
PRij 
Gij 
E3C 
CC 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Material density 
Young’s modulus in direction 𝐸𝑖. 
Elastic Poisson’s ratio 𝜈𝑖𝑗. 
Elastic shear modulus in direction 𝐺𝑖𝑗. 
Elastic compression parameter. 
Elastic compression exponent. 
TWOK 
Exponent in in-plane yield surface.
ROT 
Option for 2D-solids (shell element form 13,14,15): 
EQ.0.0:  No  rotation  of  material  axes  (default).    Direction  of
material axes are solely defined by AOPT and it is only
possible to rotate in shell-plane. 
EQ.1.0:  Rotate  coordinate  system  around  material  1-axis  such 
that 2-axis coincides with shell normal.  This rotation is 
done in addition to AOPT. 
EQ.2.0:  Rotate  coordinate  system  around  material  2-axis  such 
that 1-axis coincides with shell normal.  This rotation is
done in addition to AOPT. 
𝑖th  in-plane  plasticity  yield  parameter.    If  S0i <  0  the  absolute 
value of S0i is a curve number, see remarks.  
𝑖th in-plane plasticity hardening parameter. 
𝑖th in-plane plasticity hardening parameter. 
𝑖th in-plane plasticity hardening parameter. 
Tensile plastic Poisson’s ratio in direction 1. 
Tensile plastic Poisson’s ratio in direction 2. 
Compressive plastic Poisson’s ratio in direction 1. 
Compressive plastic Poisson’s ratio in direction 2. 
Out-of-plane plasticity yield parameter. 
Out-of-plane plasticity hardening parameter. 
Out-of-plane plasticity hardening parameter. 
Transverse shear plasticity yield parameter. 
Transverse shear plasticity hardening parameter. 
Transverse shear plasticity hardening parameter. 
S0i 
A0i 
B0i 
C0i 
PRP1 
PRP2 
PRP4 
PRP5 
ASIG 
BSIG 
CSIG 
TAU0 
ATAU 
BTAU
AOPT 
Material  axes  option  : 
EQ.0.0:  locally  orthotropic  with  material  axes  determined  by
element nodes 1, 2, and 4, as with *DEFINE_COORDI-
NATE_NODES. 
EQ.1.0:  locally orthotropic with material axes determined by a
point  in  space  and  the  global  location  of  the  element
center;  this  is  the  a-direction.    This  option  is  for  solid 
elements only. 
EQ.2.0:  globally orthotropic with material axes determined by
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0:  locally  orthotropic  material  axes  determined  by
rotating the material axes about the element normal by
an angle, BETA, from a line in the plane of the element
defined  by  the  cross  product  of  the  vector  v  with  the 
element normal. 
EQ.4.0:  locally  orthotropic  in  cylindrical  coordinate  system
with  the  material  axes  determined  by  a  vector  v,  and
an originating point, p, which define the centerline ax-
is.  This option is for solid elements only. 
LT.0.0:  the absolute value of  AOPT is a coordinate system ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
MACF 
Material axes change flag for brick elements: 
EQ.1:  No change, default, 
EQ.2:  switch material axes a and b, 
EQ.3:  switch material axes a and c, 
EQ.4:  switch material axes b and c. 
XP, YP, ZP 
Define coordinates of point 𝐩 for AOPT = 1 and 4. 
A1, A2, A3 
Define components of vector 𝐚 for AOPT = 2. 
V1, V2, V3 
Define components of vector 𝐯 for AOPT = 3 and 4. 
D1, D2, D3 
Define components of vector 𝐝 for AOPT = 2.
the element card, see *ELEMENT_SHELL_BETA or *ELEMENT_-
SOLID_ORTHO. 
*MAT_PAPER 
BETA 
Remarks: 
The stress-strain relationship for solid elements is based on a multiplicative split of the 
deformation gradient into an elastic and a plastic part 
The elastic Green strain is formed as 
𝐅 = 𝐅𝑒𝐅𝑝. 
𝐄𝑒 =
(𝐅𝑒
T𝐅𝑒 − 𝐈), 
and the 2nd Piola-Kirchhoff stress as 
𝐒 = 𝐂𝐄𝑒, 
where  the  constitutive  matrix  is  taken  as  orthotropic  and  can  be  represented  in  Voigt 
notation by its inverse as 
𝐂−1 =
𝐸1
𝜐12
𝐸1
𝜐13
𝐸1
−
−
𝜐21
𝐸2
𝐸2
𝜐23
𝐸2
−
−
𝜐31
𝐸3
𝜐32
𝐸3
𝐸3
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
. 
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
𝐺13⎦
𝐺12
𝐺23
−
−
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
In out-of-plane compression the stress is modified according to 
𝑆33 = 𝐶31𝐸11
𝑒 + 𝐶32𝐸22
𝑒 + {
𝑐 [1 − exp(−𝐶𝑐𝐸33
𝐸3
𝑒 ,
𝐸3𝐸33
𝑒 )],
𝑒 ≥ 0,
𝑒 < 0.
𝐸33
𝐸33
Three  yield  surfaces  are  present:  in-plane,  out-of-plane,  and  transverse  shear.    The  in-
plane yield surface is given as 
𝑓 = ∑
𝑖=1
⎡max(0, 𝑆: 𝑁𝑖)
⎢
𝑓 )
𝑞𝑖(𝜀𝑝
⎣
2𝑘
⎤
⎥
⎦
− 1 ≤ 0
, 
with the 6 yield plane normals (in strain Voigt notation)
𝜐1𝑝
−
√1 + 𝜐1𝑝
√1 + 𝜐1𝑝
𝑁1 =
⎡
⎢
⎣
𝑁2 =
⎡−
⎢
⎣
𝜐2𝑝
√1 + 𝜐2𝑝
√1 + 𝜐2𝑝
⎤
⎥
⎦
⎤
⎥
⎦
, 
, 
𝑁3 = [0
0 √2
𝑁4 = −
⎡
⎢
√1 + 𝜐4𝑝
⎣
−
0]
, 
𝜐4𝑝
√1 + 𝜐4𝑝
𝑁5 = −
⎡−
⎢
⎣
𝜐5𝑝
√1 + 𝜐5𝑝
√1 + 𝜐5𝑝
𝑁6 = −𝑁3. 
The yield planes describe the following states 
⎤
⎥
⎦
⎤
⎥
⎦
, 
, 
Each  hardening  function  𝑞𝑖  (note  that  𝑞6 = 𝑞3)  is  given  by  a  load  curve  if  𝑆𝑖
otherwise 
0 < 0, 
𝑞𝑖(𝜀𝑝
𝑓 ) = 𝑆𝑖
0 + 𝐴𝑖
0 tanh(𝐵𝑖
0𝜀𝑝
𝑓 ) + 𝐶𝑖
𝑓 . 
0𝜀𝑝
The out-of-plane surface is given as
𝑔 =
−𝑆33
𝑔)
𝐴𝜎 + 𝐵𝜎 exp(−𝐶𝜎𝜀𝑝
− 1 ≤ 0, 
and the transverse shear surface is 
ℎ =
√𝑆13
2 + 𝑆23
𝜏0 + [𝐴𝜏 − min(0, 𝑆33) 𝐵𝜏]𝜀𝑝
− 1 ≤ 0. 
The flow rule is given by the evolution of the plastic deformation gradient 
where the plastic velocity gradient is given as 
𝐅̇𝑝 = 𝐋𝑝𝐅𝑝, 
𝐋𝑝 =
𝑓 𝜕𝑓
𝜕𝑆11
⎡𝜀̇𝑝
⎢
⎢
𝑓 𝜕𝑓
⎢
𝜀̇𝑝
⎢
𝜕𝑆12
⎢
⎢
ℎ 𝜕ℎ
⎢
𝜀̇𝑝
𝜕𝑆13
⎣
𝑓 𝜕𝑓
𝜀̇𝑝
𝜕𝑆12
𝑓 𝜕𝑓
𝜀̇𝑝
𝜕𝑆22
ℎ 𝜕ℎ
𝜀̇𝑝
𝜕𝑆23
ℎ 𝜕ℎ
𝜀̇𝑝
𝜕𝑆13
ℎ 𝜕ℎ
𝜀̇𝑝
𝜕𝑆23
𝑔 𝜕𝑔
𝜀̇𝑝
⎤
⎥
⎥
⎥
, 
⎥
⎥
⎥
⎥
𝜕𝑆33⎦
and where it is implicitly assumed that the involved derivatives in the expression of the 
velocity gradient is appropriately normalized. 
The stress-strain relationship for shell elements is based on an additive split of the rate 
of deformation into an elastic and a plastic part 
𝐃 = 𝐃𝑒 + 𝐃𝑝, 
and the rate of Cauchy stress is given by 
𝛔̇ = 𝐂𝐃𝑒. 
In out-of-plane compression the stress rate is modified according to 
𝜎̇33 = 𝐶31𝐷11
𝑒 + 𝐶32𝐷22
𝑒 + 𝐷33
𝑒 {
𝑐 exp(−𝐶𝑐𝜀33
𝐸3
𝐸3,
𝑒 ) ,
𝑒 ≥ 0,
𝜀33
𝑒 < 0.
𝜀33
For shell elements, 𝐷33
surface 
𝑝 = 0, and only two yield surfaces are present: the in-plane yield 
𝑓 = ∑
𝑖=1
⎡max(0, 𝜎: 𝑁𝑖)
⎢
𝑓 )
𝑞𝑖(𝜀𝑝
⎣
2𝑘
⎤
⎥
⎦
− 1 ≤ 0
, 
and the transverse-shear yield surface 
ℎ =
√𝜎13
2 + 𝜎23
𝜏0 + [𝐴𝜏 − min(0, 𝜎33) 𝐵𝜏]𝜀𝑝
− 1 ≤ 0, 
and the plastic flow rule is given by
where the plastic velocity gradient is given as 
𝛆̇𝑝 = 𝐃𝑝 = 𝐋𝑝, 
𝐋𝑝 =
𝑓 𝜕𝑓
𝜕𝜎11
⎡𝜀̇𝑝
⎢
⎢
𝑓 𝜕𝑓
⎢
𝜀̇𝑝
⎢
𝜕𝜎12
⎢
⎢
ℎ 𝜕ℎ
⎢
𝜀̇𝑝
𝜕𝜎13
⎣
𝑓 𝜕𝑓
𝜀̇𝑝
𝜕𝜎12
𝑓 𝜕𝑓
𝜀̇𝑝
𝜕𝜎22
ℎ 𝜕ℎ
𝜀̇𝑝
𝜕𝜎23
ℎ 𝜕ℎ
𝜀̇𝑝
𝜕𝜎13
ℎ 𝜕ℎ
𝜀̇𝑝
𝜕𝜎23
⎤
⎥
⎥
⎥
. 
⎥
⎥
⎥
⎥
⎦
History variables: 
History variables 1 to 3 show 𝜀𝑝
𝑓 , 𝜀𝑝
𝑔 and 𝜀𝑝
ℎ, respectively.  The Effective Plastic Strain is 
𝑓 )
𝜀𝑝 = √(𝜀𝑝
𝑔)
+ (𝜀𝑝
ℎ)
+ (𝜀𝑝
*MAT_SMOOTH_VISCOELASTIC_VISCOPLASTIC 
This is Material Type 275, a smooth viscoelastic viscoplastic model based on the works 
of  Hollenstein  et.al.    [2013,  2014]  and  Jabareen  [2015].    The  stress  response  is 
rheologically represented by HJR (Hollenstein-Jabareen-Rubin) elements in parallel, see 
Figure  0-1,  where  each  element  exhibits  combinations  of  viscoelastic  and  viscoplastic 
characteristics.  The model is based on large displacement hyper-elastoplasticity and the 
numerical  implementation  is  strongly  objective,  this  together  with  the  smooth 
characteristics makes it especially suitable for implicit analysis. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
3 
K 
F 
4 
5 
6 
7 
8 
HJR  Element  Cards.    At  least  1  and  optionally  up  to  6  cards  should  be  input.    A 
keyword  card  (with  a  “*”  in  column  1)  terminates  this  input,  if  less  than  6  cards  are 
used. 
  Card 2 
Variable 
1 
A0 
Type 
F 
2 
B0 
F 
3 
A1 
F 
4 
B1 
F 
5 
M 
F 
6 
7 
8 
KAPAS 
KAPA0 
SHEAR 
F 
F 
F 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
K 
A0 
B0 
A1 
B1 
Mass density. 
Elastic bulk modulus. 
Rate dependent understress viscoplastic parameter. 
Rate independent understress plasticity parameter. 
Rate dependent overstress viscoplastic parameter. 
Rate independent overstress plasticity parameter.
𝐹 
𝐺 
𝑎0
𝑏0
𝑏1 
𝑎1
𝜅(𝜅0, 𝜅𝑠, 𝑚)
Figure 0-1.  Rheological representation of an HJR element, including the associated
parameters. 
  VARIABLE   
DESCRIPTION
Exponential hardening parameter. 
Saturated yield strain. 
Initial yield strain. 
Elastic shear modulus. 
M 
KAPAS 
KAPA0 
SHEAR 
Remarks: 
The Cauchy stress for this smooth viscoelastic viscoplastic material is given by 
𝛔 = 𝐾(𝐽 − 1)𝐈 + ∑ 𝐬𝑖
, 
𝑖=1
where 𝐾 is the elastic bulk modulus provided on the first card, 𝐽 = det(𝐅) is the relative 
volume  with  𝑭  being  the  total  deformation  gradient,  and  the  deviatoric  stresses  𝒔𝑖  are 
coming  from  the  HJR  (Hollenstein-Jabareen-Rubin)  elements  in  parallel.    Up  to  6  such 
elements can be defined for the deviatoric response and a rheological representation of 
one is shown in Figure 0-1.  Each element is associated with 8 material parameters that 
are  provided  on  the  optional  cards  and  characterize  its  inelastic  response.    All  this 
allows  for  a  wide  range  of  stress  strain  relationships  and  the  critical  part  would  be  to 
estimate  parameters  for  a  given  test  suite,  whence  some  elaboration  on  the  physical 
interpretation  of  the  individual  parameters  in  the  context  of  uniaxial  stress  is  given 
following a general description of the model. 
We  analyze  one  HJR  element  by  letting  𝐁̅̅̅̅   denote  the  associated  isochoric  elastic  left 
Cauchy-Green tensor.  Define 
The evolution of 𝐁̅̅̅̅  is given by 
𝐁̃ = 𝐁̅̅̅̅ − 1
3 𝛼𝐈,  where 𝛼 = tr(𝐁̅̅̅̅ ).
a0 = 0.0
a0 = 0.5
a0 = 1.0
a0 = 2.0
1.2
1.0
0.8
0.6
0.4
0.2
0.0
0.0
1.0
2.0
3.0
4.0
5.0
6.0
7.0
8.0
9.0
10.0
Time
Figure M275-1.  Influence of parameter 𝑎0 on stress relaxation 
𝐁̅̅̅̅̇ = 𝐋𝐁̅̅̅̅ + 𝐁̅̅̅̅ 𝐋T −
tr(𝐃)𝐁̅̅̅̅ − 𝛤̇𝐀,  where 𝐀 = 𝐁̅̅̅̅ − [
tr(𝐁̅̅̅̅ −1)
] 𝐈 
where  𝐃  is  the  rate-of-deformation  and  𝛤̇  governs  the  inelastic  deformation.    The 
functional form of 𝛤̇ is summarized in the following set of equations 
where 
𝛤̇ = 𝛤̇0 + ⟨𝑔⟩𝛤̇1 
𝛤̇𝑖 = 𝑎𝑖 + 𝑏𝑖𝜀̇,
𝑔 = 1 −
𝛾̃
𝑖 = 0,1 
⟨𝑔⟩ = max(0, 𝑔) , 
𝜀̇ = √
𝐃̃
∶ 𝐃̃ , 
𝐃̃ = 𝐃 −
tr(𝐃)𝐈, 
𝛾̃ = √
𝐁̃ ∶ 𝐁̃ , 
𝜅̇ = 𝑚𝛤̇1⟨𝑔⟩(𝜅𝑠 − 𝜅). 
A hyperelastic law with a strain energy potential for the distortional deformation given 
by
b0 =  0
b0 =  5
b0 = 25
b0 = 50
0.300
0.200
0.100
0.000
-0.100
-0.200
-0.300
-15.0
-10.0
-5.0
0.0
5.0
10.0
15.0
Strain %
Figure M275-2.  Influence of 𝑏0 in cyclic loading 
𝜓(𝛼) =
(𝛼 − 3) 
yields a contribution to the deviatoric Cauchy stress of 
𝐬 = 𝐺𝐽−1𝐁̃ . 
In uniaxial stress at constant total distortional rate of deformation ±𝜀̇ (tension or 
compression), these equations can be reduced to scalar correspondents 
𝑏̅
𝑏̅
= 2
⎜⎜⎛±𝜀̇ − 𝛤̇
⎝
𝑏̅√𝑏̅ − 1
⎟⎟⎞ 
2𝑏̅√𝑏̅ + 1⎠
𝜏 = 𝐺
⎜⎛𝑏̅ −
⎝
⎟⎞
√𝑏̅⎠
(M275.1)
where  𝑏̅  is  the  component  of  𝑩̅̅̅̅̅  in  the  direction  of  deformation  and  𝜏  is  the  uniaxial 
Kirchhoff stress.  The evolution of 𝛤  follows the equations above with 
𝛾̃ = 1
2 ∣𝑏̅ − 1/√𝑏̅∣. 
Even  though  analytical  solutions  may  be  out  of  reach,  this  would  be  the  basis  for 
estimating  as  well  as  interpreting  the  material  parameters.    Obviously  the  shear 
modulus  𝐺  (SHEAR)  provides  the  elastic  deviatoric  stiffness,  for  a  purely  elastic 
material  just  define  one  such  parameter  and  leave  out  all  the  other  parameters  on  the 
same card.  If several cards are used, the effective elastic shear stiffness is the sum of the 
2-1404 (MAT_248)
0.07
0.05
0.02
0.00
-0.03
-0.05
-0.08
b1 =  100
b1 =  200
b1 =  500
b1 = 1000
0.0
0.5
1.0
1.5
2.0
2.5
3.0
3.5
4.0
4.5
5.0
Strain %
Figure M275-3.  Effect of 𝑏1 in cyclic loading 
contributions from each of the corresponding HJR elements.  An interesting observation 
is that the stress in a HJR element saturates to a value given by the solution of 𝑏̅ to 
𝑏̅√𝑏̅ (±2 − {𝑏0 + 𝑏1 +
𝑎0 + 𝑎1
𝜀̇
}) ± 2√𝑏̅𝜅𝑠 (𝑏1 +
)
𝑎1
𝜀̇
𝑎0 + 𝑎1
𝜀̇
+ (±1 + {𝑏0 + 𝑏1 +
}) = 0 
(M275.2)
in  tension  (+)  and  compression  (−),  followed  by  application  of  (M275.1)  above,  this 
assuming that 
in tension 
𝑏0 + 𝑏1 +
𝑎0 + 𝑎1
𝜀̇
> 2 
𝑏0 + 𝑏1 +
𝑎0 + 𝑎1
𝜀̇
> 1 
in compression.  This expression will be utilized in special cases below when examining 
each inelastic material parameter individually, the material parameters above are input 
on the HJR element cards as A0, B0, A1, B1 and KAPAS. 
A  Maxwell  material  is  obtained  by  providing  an  element  with  a  nonzero  𝑎0  (A0)  and 
other  parameters  zero,  this  parameter  should  be  interpreted  as  the  viscoelastic 
relaxation  coefficient  determining  the  rate  at  which  the  stress  relaxes  to  zero,  see 
parameter  BETA  in  *MAT_VISCOELASTIC.    In  Figure  M275-1  a  stress  relaxation  is 
shown for a strain controlled problem using two HJR elements and normalized material 
parameters  using  a  bulk  modulus  of  𝐾 = 1.    For  the  first  element  𝐺 = 0.5  and  for  the
other  𝐺 = 1  and    𝑎0  varies,  all  other  parameters  are  zero.    The  engineering  strain  is 
ramped to 50% from 𝑡 = 0 to 𝑡 = 1 and then kept constant, the response is very similar 
to other viscoelastic models in LS-DYNA.  Not surprisingly, a HJR element with 𝑎0 > 0 
(and  𝑎1 = 𝑏1 = 0)  will  always  relax  to  zero  stress,  which  follows  from  (M275.1)  and 
(M275.2), thus the relaxed stress in this case comes from the purely elastic element.  A 
general  viscoelastic  material  can  be  obtained  by  putting  several  such  HJR  elements  in 
parallel, in analogy to *MAT_GENERAL_VISCOELASTIC. 
For a nonzero 𝑏0 (B0) and other parameters zero, a rate independent plastic response is 
obtained  exhibiting  zero  yield  stress,  i.e.,  inelastic  strains  develop  immediately  upon 
loading.    From  (M275.2)  the  value  of  𝑏0  determines  the  saturated  stress  value  for  the 
associated HJR element by (M275.1) and 
𝑏̅ = (
𝑏0 ± 1
𝑏0 ∓ 2
2/3
)
in tension (+) and compression (−), respectively.  A smooth response is obtained that is 
characterized by hysteresis as shown in Figure M275-2.  The same material parameters 
as in the previous example is used with the exception of varying 𝑏0 with vanishing 𝑎0.  
The  deformation  is  controlled  by  a  cyclic  Cauchy  stress  between  −0.25  and  0.25,  for 
larger 𝑏0 a hysteresis is observed.  It should however be mentioned that the hysteresis 
vanishes  as  𝑏0 → ∞  as  the  stress  for  the  second  element  saturates  quickly  to  a  small 
value, so it is not trivial to quantitatively estimate the amount of hysteresis for a given 
parameter setting and deformation.
0.07
0.05
0.02
0.00
-0.03
-0.05
-0.08
m = 0.1
m = 0.2
m = 0.5
m = 1.0
0.0
0.5
1.0
1.5
2.0
2.5
3.0
3.5
4.0
4.5
5.0
Strain %
Figure  M275-4.    Softening  response  in  cyclic  loading  for  various  values
of 𝑚 
Rate independent plasticity with a nonzero yield stress can be obtained by a nonzero 𝑏1 
(B1)  in  combination  with  parameters 𝜅0  (KAPA0),   𝜅𝑠  (KAPAS)  and  𝑚  (M).    The  yield 
stress in the sense of von Mises is given by 
𝜎𝑌 = 2𝐺𝐽−1𝜅 
and whence 𝜅 is interpreted as the current yield strain.  Here 𝑏1 determines the amount 
of  overstress  through  (M275.1)  and  (M275.2),  requiring  the  solution  of  a  non-trivial 
polynomial equation.  This is exemplified in Figure M275-3 using one HJR element with 
𝐾 = 1, 𝐺 = 1.5,  𝜅0 = 𝜅𝑠 = 0.01  and  𝑚 = 0.    The  engineering  strain  is  ramped  up  to  5% 
and down to 0 and 𝑏1 is varied with all other parameters zero, the response tends to an 
elastic-perfectly  plastic  as  𝑏1  increases.    The  saturated  stress  value  for  𝑏1 → ∞  can  be 
calculated as 
𝑏̅ =
⎡
⎜⎜⎛1
⎢⎢
⎝
⎣
+ √
∓
8𝜅𝑠
27
⎟⎟⎞
⎠
1/3
+
⎜⎜⎛1
⎝
− √
∓
8𝜅𝑠
27
⎟⎟⎞
⎠
1/3
⎤
⎥⎥
⎦
(M275.3)
and employing (M275.1). 
Isostropic strain hardening 𝜅𝑠 > 𝜅0 or softening 𝜅𝑠 < 𝜅0 is obtained with 𝑚 > 0, 𝜅 tends 
exponentially  towards  𝜅𝑠  at  a  rate  determined  by  𝑚.    Using  𝑏1 = 1000,  i.e.,  very  little 
overstress,  𝜅0 = 0.02, 𝜅𝑠 = 0.01 and varying 𝑚 the softening response in Figure M275-4 
is  obtained.    The  rate  at  which  the  element  hardens  is  difficult  to  quantitatively 
estimate,  but  presumably  it  depends  not  only  on  𝑚  but  also  on  𝑏1.    It  is  important  to 
note  however  that  for  small  to  moderate  𝑏1  the  model  appears  to  harden  with  𝑚 = 0,
de/dt =  0.2
de/dt =  4.0
de/dt = 10.0
de/dt = 20.0
0.125
0.100
0.075
0.050
0.025
0.000
-0.025
-0.050
-0.075
0.0
0.5
1.0
1.5
2.0
2.5
3.0
3.5
4.0
4.5
5.0
Strain %
Figure M275-5.  Strain rate dependence for 𝑎1 = 1000 and 𝑏1 = 10 
which is due to larger overstress.  The hardening determined by 𝑚 can be determined 
from  a  loading,  unloading  and  reloading  cycle  to  detect  how  the  the  yield  strain  𝜅 
changes, see Hollenstein et.al.  [2013]. 
Finally, 𝑎1 (A1) is the viscoplastic parameter determining how stress responds to change 
in  strain  rate.    Its  interpretation  is  very  similar  to  that  of  𝑎0,  stress  increases  with 
increasing loading rate and relaxes to the saturated stress value given by (M275.1) and 
(M275.2).    In  Figure  M275-5  a  rate  dependency  is  illustrated  for  𝐾 = 1, 𝐺 = 1.5, 
𝜅0 = 𝜅𝑠 = 0.01  and  𝑚 = 0,  where  we  have  put 𝑎1 = 1000  and  𝑏1 = 10.    The  engineering 
strain  rate  varies  from  0.2  to  20  and  for  small  strain  rates  (M275.3)  can  be  used  for 
estimating the saturated stress, but in general (M275.2) must be used. 
Putting several HJR elements in parallel can thus provide a fairly general combination 
of viscoelastic/viscoplastic response with isotropic hardening/softening, but this of 
course requires a rich test suite and a good way of estimating the material parameters.  
Presumably it is often sufficient to neglect some effects and work with only a subset of 
the material parameters. 
For post-processing, the effective plastic strain in this model is defined as 
where 
𝜀𝑝 = √
𝛆𝑝 ∶ 𝛆𝑝 
𝛆𝑝 = 𝛆𝑡 − 𝛆𝑒
is a crude estimation of the difference between total and elastic strain.  We set 
where 
𝛆𝑡 =
2𝐽
[𝐁 −
tr(𝐁)𝐈] 
𝛆𝑒 =
2𝐺
[𝛔 −
tr(σ)𝐈] 
𝐁 = 𝐽−2/3𝐅𝐅T 
and 𝐺 here is the sum of all shear moduli defined on the HJR element cards.  Note that 
this does not correspond to the traditional measure of effective plastic strain which 
should be accounted for when validating results.
*MAT_CHRONOLOGICAL_VISCOELASTIC 
This is Material Type 276.  This material model provides a general viscoelastic Maxwell 
model  having  up  to  6  terms  in  the  prony  series  expansion  and  is  useful  for  modeling 
dense  continuum  rubbers  and  solid  explosives.    It  is  similar  to  Material  Type  76  but 
allows  the  incorporation  of  aging  effects  on  the  material  properties.    Either  the 
coefficients  of  the  prony  series  expansion  or  a  relaxation  curve  may  be  specified  to 
define the viscoelastic deviatoric and bulk behavior. 
The  material  model  can  also  be  used  with  laminated  shell.    Either  an  elastic  or 
viscoelastic layer can be defined with the laminated formulation.  To activate laminated 
shell  you  need  the  laminated  formulation  flag  on  *CONTROL_SHELL.    With  the 
laminated option a user defined integration rule is needed. 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
4 
BULK 
PCF 
Type 
A8 
F 
F 
F 
5 
EF 
F 
6 
TREF 
F 
7 
A 
F 
8 
B 
F 
If fitting is done from a relaxation curve, specify fitting parameters on card 2, otherwise
if constants are set on Viscoelastic Constant Cards LEAVE THIS CARD BLANK. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
NT 
BSTART 
TRAMP 
LCIDK 
NTK 
BSTARTK  TRAMPK 
Type 
F 
I 
F 
F 
F 
I 
F
Viscoelastic Constant Cards.  Up to 12 cards may be input.  A keyword card (with a 
“*” in column 1) terminates this input if less than 12 cards are used.  These cards are not 
needed if relaxation data is defined.  The number of terms for the shear behavior may 
differ from that for the bulk behavior: simply insert zero if a term is not included.  If an 
elastic layer is defined you only need to define GI and KI (note in an elastic layer only 
one card is needed). 
 Optional 
Variable 
Type 
1 
GI 
F 
2 
BETAI 
F 
3 
KI 
F 
  VARIABLE   
MID 
4 
5 
6 
7 
8 
BETAKI 
F 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density. 
BULK 
Elastic bulk modulus. 
PCF 
EF 
TREF 
A 
B 
LCID 
NT 
Tensile pressure elimination flag for solid elements only.  If set to
unity tensile pressures are set to zero. 
Elastic  flag  (if  equal  1,  the  layer  is  elastic.    If  0  the  layer  is
viscoelastic). 
Reference  temperature  for  shift  function  (must  be  greater  than 
zero). 
Chronological coefficient 𝛼(𝑡𝑎). See Remarks below. 
Chronological coefficient 𝛽(𝑡𝑎). See Remarks below. 
Load curve ID for deviatoric behavior if constants, Gi, and βi are 
determined via a least squares fit.  This relaxation curve is shown
below. 
Number of terms in shear fit.  If zero the default is 6.  Fewer than
NT  terms  will  be  used  if  the  fit  produces  one  or  more  negative
shear moduli.  Currently, the maximum number is set to 6.
BSTART 
*MAT_CHRONOLOGICAL_VISCOELASTIC 
DESCRIPTION
In the fit, 𝛽1  is set to zero, 𝛽2  is set to BSTART, 𝛽3  is 10 times 𝛽2, 
𝛽4 is 10 times 𝛽3 , and so on.  If zero, BSTART is determined by an
iterative trial and error scheme. 
TRAMP 
Optional ramp time for loading. 
LCIDK 
Load  curve  ID  for  bulk  behavior  if  constants,  𝐾𝑖,  and  𝛽𝐾𝑖    are 
determined via a least squares fit.  This relaxation curve is shown
below. 
NTK 
Number  of  terms  desired  in  bulk  fit.    If  zero  the  default  is  6.
Currently, the maximum number is set to 6. 
BSTARTK 
In  the  fit,  Β𝐾1    is  set  to  zero,  Β𝐾2    is  set  to  BSTARTK,  𝛽𝐾3    is  10 
times 𝛽𝐾2,    is 𝛽𝐾4 10 times 𝛽𝐾3 , and so on.  If zero, BSTARTK is 
determined by an iterative trial and error scheme. 
TRAMPK 
Optional ramp time for bulk loading. 
Gi 
Optional shear relaxation modulus for the ith term 
BETAi 
Optional shear decay constant for the ith term 
Ki 
Optional bulk relaxation modulus for the ith term 
BETAKi 
Optional bulk decay constant for the ith term 
Remarks: 
The Cauchy stress, 𝜎𝑖𝑗, is related to the strain rate by  
𝜎𝑖𝑗(𝑡) = −𝑝𝛿𝑖𝑗 + ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)
∂𝜀𝑘𝑙(𝜏)
∂𝜏
𝑑𝜏
For  this  model,  it  is  postulated  that  the  mathematical  form  is  preserved  in  the 
′ (𝑡𝑎, 𝑡) 
constitutive equation for aging; however two new material functions, 𝑔0
are introduced to replace 𝑔0 and 𝑔1(𝑡), which is expressed in terms of a Prony series as 
in  material  model  76,  *MAT_GENERAL_VISCOELASTIC.    The  aging  time  is  denoted 
by 𝑡𝑎. 
′ (𝑡𝑎) and 𝑔1
𝜎𝑖𝑗(𝑡𝑎, 𝑡) = −𝑝𝛿𝑖𝑗 + ∫ 𝑔𝑖𝑗𝑘𝑙
′ (𝑡𝑎, 𝑡 − 𝜏)
∂𝜀𝑘𝑙(𝜏)
∂𝜏
𝑑𝜏
where 
′ (𝑡𝑎, 𝑡) = 𝛼(𝑡𝑎)𝑔𝑖𝑗𝑘𝑙[𝛽(𝑡𝑎)𝑡] 
𝑔𝑖𝑗𝑘𝑙
where  𝛼(𝑡𝑎)  and  𝛽(𝑡𝑎)  are  two  new  material  properties  that  are  functions  of  the  aging 
time 𝑡𝑎.  The material properties functions 𝛼(𝑡𝑎) and 𝛽(𝑡𝑎) will be determined  with the 
experimental results.  For determination of 𝛼(𝑡𝑎) and 𝛽(𝑡𝑎), Eq.  (2) can be written in the 
following form 
log(𝜎𝑖𝑗 − 𝑝𝛿𝑖𝑗)
= log𝛼(𝑡𝑎) + log(𝜎𝑖𝑗 − 𝑝𝛿𝑖𝑗)
𝑡𝑎=0,𝑡→𝜉
𝑡𝑎,𝑡
log𝜉 = log𝛽(𝑡𝑎) + log𝑡 
Therefore,  if  one  plots  the  stress  versus  time  on  log-log  scales,  with  the  vertical  axis 
being the stress and the horizontal axis being the time, then the stress-relaxation curve 
for  any  aged  time  history  can  be  obtained  directly  from  the  stress-relaxation  curve  at 
𝑡𝑎 = 0 by imposing a vertical shift and a horizontal shift on the stress-relaxation curves.  
The vertical shift and the horizontal shift are log𝛼(𝑡𝑎) and log𝛽(𝑡𝑎) respectively.
*MAT_ADHESIVE_CURING_VISCOELASTIC 
This is Material Type 277.  It is useful for modeling adhesive materials during chemical 
curing.  This material model provides a general viscoelastic Maxwell model having up 
to  16  terms  in  the  Prony  series  expansion.    It  is  similar  to  Material  Type  76,  but  the 
viscoelastic  properties  do  not  only  depend  on  the  temperature  but  also  on  an  internal 
variable  representing  the  state  of  cure  for  the  adhesive.    The  kinematic  of  the  curing 
process depends on temperature as well as on temperature rate and follows the Kamal 
model. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
K1 
F 
3 
4 
K2 
F 
4 
5 
C1 
F 
5 
Variable 
CHEXP1 
CHEXP2 
CHEXP3  LCCHEXP LCTHEXP
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
I 
4 
I 
5 
6 
C2 
F 
6 
R 
F 
6 
7 
M 
F 
7 
8 
N 
F 
8 
TREFEXP 
DOCREFE
XP 
F 
7 
F 
8 
Variable  WLFTREF  WLFA 
WLFB 
LCG0 
LCK0 
IDOC 
INCR 
Type 
F 
F 
F 
I 
I 
F 
I 
Viscoelastic Constant Cards.  Up to 16 cards may be input.  A keyword card (with a 
“*”  in  column  1)  terminates  this  input  if  less  than  16  cards  are  used.    The  number  of 
terms  for  the  shear  behavior  may  differ  from  that  for  the  bulk  behavior:  simply  insert 
zero if a term is not included.   
 Optional 
Variable 
Type 
1 
GI 
F 
2-1414 (MAT_248) 
2 
BETAGI 
F 
3 
KI 
F 
4 
5 
6 
7 
8 
BETAKI
VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
K1 
K2 
C1 
C2 
M 
N 
Mass density. 
Parameter 𝑘1 for Kamal model.  
Parameter 𝑘2 for Kamal model. 
Parameter 𝑐1 for Kamal model.  
Parameter 𝑐2 for Kamal model.  
Exponent 𝑚 for Kamal model 
Exponent 𝑛 for Kamal model. 
CHEXP1 
CHEXP2 
CHEXP3 
LCCHEXP 
LCTHEXP 
R 
TREFEXP 
DOCREFEXP 
Quadratic parameter 𝛾2 for chemical shrinkage. 
Linear parameter 𝛾1 for chemical shrinkage. 
Constant parameter 𝛾0 for chemical shrinkage. 
Load  curve  ID  to  define  the  coefficient  for  chemical  shrinkage
𝛾(𝛼)  as  a  function  of  the  state  of  cure  𝛼.    If  set,  parameters 
CHEXP1, CHEXP2 and CHEXP3 are ignored. 
Load  curve  ID  or  table  ID  defining  the  instantaneous  coefficient
of  thermal  expansion 𝛽(𝛼, 𝑇)  as  a  function  of  cure  𝛼  and 
temperature  𝑇.    If  referring  to  a  load  curve,  parameter  𝛽(𝑇)  is  a 
function of temperature 𝑇. 
Gas constant 𝑅 for Kamal model. 
Reference  temperature  𝑇0  for  secant  form  of  thermal  expansion. 
See Remarks below. 
Reference  degree  of  cure  𝛼0  for  sequential  form  of  chemical 
expansion.  See Remarks below. 
WLFTREF 
Reference temperature for WLF shift function. 
WLFA 
WLFB 
Parameter 𝐴 for WLF shift function. 
Parameter 𝐵 for WLF shift function.
*MAT_ADHESIVE_CURING_VISCOELASTIC 
DESCRIPTION
LCG0 
LCK0 
IDOC 
INCR 
Load curve ID defining the instantaneous shear modulus 𝐺0 as a 
function of state of cure. 
Load  curve  ID  defining  the  instantaneous  bulk  modulus  𝐾0 as  a 
function of state of cure. 
Initial degree of cure. 
Switch between incremental and total stress formulation. 
EQ.0: total form:  (DEFAULT) 
EQ.1:  incremental form: (recommended) 
GI 
Shear relaxation modulus for the ith term for fully cured material.
BETAGI 
Shear decay constant for the ith term for fully cured material. 
KI 
Bulk relaxation modulus for the ith term for fully cured material. 
BETAKI 
Bulk decay constant for the ith term for fully cured material. 
Remarks: 
Within  this  material  formulation  an  internal  variable 𝛼  has  been  included  to  represent 
the degree of cure for the adhesive.  The evolution equation for this variable is given by 
the Kamal model and reads 
dα
dt
= (𝑘1  exp (
−𝑐1
𝑅𝑇
) + 𝑘2  exp (
−𝑐2
𝑅𝑇
) 𝛼𝑚) (1 − 𝛼)𝑛 
The chemical reaction of the curing process results in a shrinkage of the material.  The 
coefficient of the chemical shrinkage 𝛾(𝛼) can either be given by a load curve or using 
the quadratic expression  
𝛾(𝛼) = 𝛾2𝛼2 + 𝛾1𝛼 + 𝛾0 
For  non-negative  values  of  the  reference  degree  of  cure  𝛼0,  a  secant  form  is  used  to 
compute the chemical strains 
Otherwise a differential form is used: 
𝜀𝑐ℎ = 𝛾(𝛼)(𝛼 − 𝛼0) − 𝛾(𝛼𝐼)(𝛼𝐼 − 𝛼0) 
𝑑𝜀𝑐ℎ = 𝛾(𝛼)𝑑𝛼  
Analogously,  the  thermal  strains  are  either  defined  in  a  secant  or  differential  form, 
depending  on  the  reference  temperature    𝑇0.    In  both  cases  the  coefficient  of  thermal 
expansion can be given as 2d table depending on degree of cure and temperature. 
Finally, the Cauchy stress, 𝜎𝑖𝑗, is related to the strain rate by
𝜎𝑖𝑗(𝑡) = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)
∂𝜀𝑘𝑙(𝜏)
∂𝜏
𝑑𝜏
The relaxation functions 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) are represented in this material formulation by up to 
16 terms (not including the instantaneous modulus 𝐺0) of the Prony series: 
g(𝑡, 𝛼) = 𝐺0(𝛼) − ∑ 𝐺𝑖(𝛼)
+ ∑ 𝐺𝑖(𝛼)
𝑒−𝛽𝑖𝑡 
For  the  sake  of  simplicity,  a  constant  ratio  𝐺𝑖(𝛼) 𝐺0(𝛼)
  for  all  degrees  of  cure  is 
assumed.  Consequently, it suffices to define one term 𝐺0(𝛼) as a function of the degree 
of cure and further coefficients for the fully cured state of the adhesive: 
⁄
g(𝑡, 𝛼) = 𝐺0(𝛼)
⎜⎜⎛1 − ∑
⎝
𝐺𝑖,𝛼=1.0
𝐺0,𝛼=1.0
(1 − 𝑒−𝛽𝑖𝑡)
⎟⎟⎞ 
⎠
A possible temperature effect on the stress relaxation is accounted for by the Williams-
Landau-Ferry  (WLF)  shift  function.    For  details  on  this  function,  please  see  material 
formulation 76, *MAT_GENERAL_VISCOELASTIC.
*MAT_CF_MICROMECHANICS 
This is Material Type 278 developed for draping and curing analysis of prepreg carbon 
fiber sheets.  This material model is mixture of MAT_234 and MAT_277, with MAT_234 
providing reorientation and locking phenomenon of fibers and MAT_277 providing the 
viscoelastic behavior of epoxy resin.  The overall stress has contribution from both fiber 
orientation and deformation and epoxy resin.  
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
E1 
F 
3 
4 
E2 
F 
4 
5 
6 
G12 
G23 
F 
5 
Variable 
EKA 
EUA 
VMB 
EKB 
THL 
Type 
F 
  Card 3 
Variable 
Type 
1 
W 
F 
F 
2 
F 
3 
SPAN 
THICK 
F 
F 
  Card 4 
1 
Variable 
AOPT 
Type 
2 
A1 
F 
3 
A2 
F 
F 
4 
H 
F 
4 
A3 
F 
F 
5 
AREA 
F 
5 
7 
EU 
F 
7 
8 
C 
F 
8 
THI1 
THI2 
F 
7 
F 
8 
F 
6 
TA 
F 
6 
6 
7
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
4 
D1 
F 
5 
D2 
F 
6 
D3 
F 
*MAT_278 
7 
8 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VYARN 
Type 
F 
  Card 6 
Variable 
1 
K1 
Type 
F 
2 
K2 
F 
3 
C1 
F 
4 
C2 
F 
5 
M 
F 
  Card 7 
1 
2 
3 
4 
5 
Variable 
EXP1 
CHEXP2 
CHEXP3 
LCCHEX  LCTHEXP0
Type 
F 
  Card 8 
1 
F 
2 
F 
3 
F 
4 
F 
5 
6 
N 
F 
6 
R 
F 
6 
7 
8 
7 
8 
TREFEXP  ALPREEXP
F 
7 
F 
8 
Variable  WLFTREF  WLFA 
WLFB 
LCG0 
LCBULK0
IDOC 
XINCRM 
Type 
F 
F 
F 
F 
F 
F
Viscoelastic Constant Cards.  Up to 14 cards may be input.  A keyword card (with a 
“*”  in  column  1)  terminates  this  input  if  less  than  14  cards  are  used.    The  number  of 
terms  for  the  shear  behavior  may  differ  from  that  for  the  bulk  behavior:  simply  insert 
zero if a term is not included.   
  Card 8 
Variable 
Type 
1 
GI 
F 
2 
BETAGI 
F 
3 
KI 
F 
4 
5 
6 
7 
8 
BETAKI 
F 
 VARIABLE  
DESCRIPTION
MID 
RO 
E1 
E2 
G12 
G23 
EU 
C 
EKA 
EUA 
VMB 
Ekb 
THL 
TA 
THI1 
THI2 
W 
SPAN 
THICK 
H 
Material identification.  A unique number or label not exceeding 
8 characters must be specified. 
Mass density. 
𝐸1, Young’s modulus in the yarn axial-direction. 
𝐸2, Young’s modulus in the yarn transverse-direction. 
𝐺12, Shear modulus of the yarns. 
transverse shear modulus. 
Ultimate strain at failure. 
Coefficient of friction between the fibers. 
Elastic constant of element "a". 
Ultimate strain of element "a". 
Damping coefficient of element "b". 
Elastic constant of element "b" 
Yarn locking angle. 
Transition angle to locking. 
Initial braid angle 1. 
Initial braid angle 2. 
Fiber width. 
Span between the fibers. 
Real fiber thickness. 
Effective fiber thickness.
VARIABLE  
DESCRIPTION
AREA 
APOT 
VYARN 
K1 
K2 
C1 
C2 
M 
N 
CHEXP1 
CHEXP2 
CHEXP3 
LCCHEXP 
LCTHEXP 
R 
TREFEXP 
DOCREFEXP 
Fiber cross-sectional area. 
Material  axes  option  . 
Volume fraction of yarn 
Parameter 𝑘1 for Kamal model.  
Parameter 𝑘2 for Kamal model. 
Parameter 𝑐1 for Kamal model.  
Parameter 𝑐2 for Kamal model.  
Exponent 𝑚 for Kamal model 
Exponent 𝑛 for Kamal model. 
Quadratic parameter 𝛾2 for chemical shrinkage. 
Linear parameter 𝛾1 for chemical shrinkage. 
Constant parameter 𝛾0 for chemical shrinkage. 
Load  curve  ID  to  define  the  coefficient  for  chemical  shrinkage 
𝛾(𝛼)  as  a  function  of  the  state  of  cure  𝛼.    If  set,  parameters 
CHEXP1, CHEXP2 and CHEXP3 are ignored. 
Load curve ID or table ID defining the instantaneous coefficient 
of  thermal  expansion 𝛽(𝛼, 𝑇)  as  a  function  of  cure  𝛼  and 
temperature 𝑇.  If referring to a load curve, parameter 𝛽(𝑇) is a 
function of temperature 𝑇. 
Gas constant 𝑅 for Kamal model. 
Reference temperature 𝑇0 for secant form of thermal expansion. 
Reference  degree  of  cure  𝛼0  for  sequential  form  of  chemical 
expansion.  
WLFTREF 
Reference temperature for WLF shift function. 
WLFA 
WLFB 
LCG0 
LCK0 
Parameter 𝐴 for WLF shift function. 
Parameter 𝐵 for WLF shift function. 
Load curve ID defining the instantaneous shear modulus 𝐺0 as a 
function of state of cure. 
Load curve ID defining the instantaneous bulk modulus 𝐾0 as a 
function of state of cure. 
IDOC 
Initial degree of cure.
*MAT_CF_MICROMECHANICS 
DESCRIPTION
INCR 
Switch between incremental and total stress formulation. 
EQ.0: total form:  (DEFAULT) 
EQ.1:  incremental form: (recommended) 
GI 
Shear  relaxation  modulus  for  the  ith  term  for  fully  cured 
material. 
BETAGI 
Shear decay constant for the ith term for fully cured material. 
KI 
Bulk relaxation modulus for the ith term for fully cured material. 
BETAKI 
Bulk decay constant for the ith term for fully cured material.
*MAT_279 
This is material type 279.  This is a cohesive model for paper materials and can be used 
only with cohesive element fomulations; see the variable ELFORM in *SECTION_SOL-
ID and *SECTION_SHELL. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
RO 
ROFLG 
INTFAIL 
EN0 
ET0 
EN1 
ET1 
Type 
A8 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 2 
1 
Variable 
T0N 
2 
DN 
3 
4 
T1N 
T0T 
Type 
F 
F 
F 
F 
5 
DT 
F 
6 
7 
T1T 
E3C 
F 
F 
8 
CC 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ASIG 
BSIG 
CSIG 
FAILN 
FAILT 
Type 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
RO 
Mass density
ROFLG 
Flag for whether density is specified per unit area or volume. 
ROFLG.EQ.0:  specified density per unit volume (default) 
ROFLG.EQ.1:  specifies  the  density 
is  per  unit  area  for
controlling  the  mass  of  cohesive  elements  with
an initial volume of zero. 
INTFAIL 
The  number  of  integration  points  required  for  the  cohesive
element to be deleted.  If it is zero, the element will not be deleted
even if it satisfies the failure criterion.  The value of INTFAIL may
range from 1 to 4, with 1 the recommended value. 
EN0 
EN1 
ET0 
ET1 
T0N 
DN 
T1N 
T0T 
DT 
T1T 
E3C 
CC 
ASIG 
BSIG 
The initial tensile stiffness (units of stress / length) normal to the 
plane of the cohesive element. 
The  final  tensile  stiffness  (units  of  stress / length)  normal  to  the 
plane of the cohesive element. 
The  initial  stiffness  (units  of  stress / length)  tangential  to  the 
plane of the cohesive element.  
The final stiffness (units of stress / length) tangential to the plane 
of the cohesive element. 
Peak tensile traction in normal direction. 
Scale factor (unit of length). 
Final tensile traction in normal direction. 
Peak  tensile  traction  in  tangential  direction.    If  negative,  the
absolute  value  indicates  a  curve  with  respect  to  the  normal
traction. 
Scale  factor  (unit  of  length).    If  negative,  the  absolute  value 
indicates a curve with respect to the normal stress. 
Final  traction  in  tangential  direction.    If  negative,  the  absolute
value indicates a curve with respect to the normal traction. 
Elastic parameter in normal compression. 
Elastic parameter in normal compression. 
Plasticity hardening parameter in normal compression. 
Plasticity hardening parameter in normal compression.
𝑇 
𝑇0
𝐸0 
𝐸(𝛿 ̅
𝑝)
𝑇1
Figure M279-1.  Traction-separation law 
CSIG 
Plasticity hardening parameter in normal compression. 
Maximum  effective  separation  distance  in  normal  direction. 
Beyond this distance failure occurs. 
Maximum  effective  separation  distance  in  tangential  direction. 
Beyond this distance failure occurs. 
FAILN 
FAILT 
Remarks: 
In  this  elastoplastic  cohesive  material  the  normal  and  tangential  directions  are  treated 
separately,  but  can  be  connected  by  expressing  the  in-plane  traction  parameters  as 
functions  of  the  normal  traction.    In  the  normal  direction  the  material  uses  different 
models in tension and compression. 
Normal tension: 
Assume the total separation is an additive split of the elastic and plastic separation 
𝛿 = 𝛿𝑒 + 𝛿𝑝 . 
In normal tension (𝛿𝑒 > 0) the elastic traction is given by 
𝑇 = 𝐸𝛿𝑒 = 𝐸(𝛿 − 𝛿𝑝) ≥ 0, 
where the tensile normal stiffness 
𝐸 = (𝐸𝑁
0 − 𝐸𝑁
1 ) exp
−𝛿 ̅
𝛿𝑁 ⎠
⎟⎞ + 𝐸𝑁
1  , 
⎜⎛
⎝
depends on the effective plastic separation in the normal direction
Yield traction for tensile loads in normal direction is given by 
𝛿 ̅
𝑝 = ∫∣d𝛿𝑝∣ . 
𝑇yield = (𝑇𝑁
0 − 𝑇𝑁
1 ) exp
⎜⎛
⎝
−𝛿 ̅
𝛿𝑁 ⎠
⎟⎞ + 𝑇𝑁
1 ≥ 0, 
and  yielding  occurs  when  𝑇 > 𝑇yield ≥ 0.  The  above  elastoplastic  model  gives  the 
traction-separation law depicted in Figure M279-1. 
Normal compression: 
In normal compression the elastic traction is 
and the yield traction is 
𝑇 = 𝐸3
𝑐 [1 − exp(−𝐶𝑐𝛿𝑒)] ≤ 0, 
𝑇yield = −[𝐴𝜎 + 𝐵𝜎 exp(−𝐶𝜎𝛿 ̅
𝑝)] ≤ 0, 
with yielding if 𝑇 < 𝑇yield ≤ 0. 
Tangential traction: 
Assume  the  total  separation  is  an  additive  split  of  the  elastic  and  plastic  separation  in 
each in-plane direction 
The elastic traction is given by 
𝛿𝑖 = 𝛿𝑒
𝑖 ,
𝑖 + 𝛿𝑝
𝑖 = 1,2. 
where the tensile normal stiffness 
𝑇𝑖 = 𝐸𝛿𝑒
𝑖 = 𝐸(𝛿𝑖 − 𝛿𝑝
𝑖 ), 
𝐸 = (𝐸𝑇
0 − 𝐸𝑇
1 ) exp
−𝛿 ̅
𝛿𝑇 ⎠
⎟⎞ + 𝐸𝑇
1 , 
⎜⎛
⎝
depends on the effective plastic separation 
𝛿 ̅
𝑝 = ∫ d𝛿𝑝 ,
d𝛿𝑝 = √(d𝛿𝑝
1)
2)
+ (d𝛿𝑝
. 
Yield traction is given by 
𝑇yield = (𝑇𝑇
0 − 𝑇𝑇
⎜⎛
1 ) exp 
⎝
−𝛿 ̅
𝛿𝑇 ⎠
⎟⎞ + 𝑇𝑇
1 , 
and yielding occurs when  
2 + 𝑇2
𝑇1
2 − 𝑇𝑦𝑖𝑒𝑙𝑑
2 ≥ 0. 
The plastic flow increment follows the flow rule
d𝛿𝑝
𝑖 =
𝑇𝑖
2 + 𝑇2
√𝑇1
d𝛿𝑝. 
The  above  elastoplastic  model  gives  the  traction-separation  law  depicted  in  Figure 
M279-1. 
History variables 
This material uses five history variables.  Effective separation in the tangential direction 
is  saved  as  Effective  Plastic  Strain.    History  variable  1  and  2  indicates  the  plastic 
separation  in  each  tangential  direction.    Effective  plastic  separation  and  plastic 
separation in the normal direction are saved as history variable 3 and 4, respectively.
*MAT_GLASS 
This is Material Type 280.  It is a smeared fixed crack model with a selection of different 
brittle,  stress-state  dependent  failure  criteria  such  as  Rankine,  Mohr-Coulomb,  or 
Drucker-Prager.    The  model  incorporates  up  to  2  (orthogonal)  cracks  per  integration 
point,  simultaneous  failure  over  element  thickness,  and  crack  closure  effects.    It  is 
available for shell elements and explicit analysis only. 
  Card 1 
1 
Variable 
MID 
2 
RO 
Type 
A8 
F 
  Card 2 
1 
Variable 
FMOD 
Type 
F 
  Card 3 
1 
2 
FT 
F 
2 
3 
E 
F 
3 
FC 
F 
3 
4 
PR 
F 
4 
AT 
F 
4 
5 
6 
7 
8 
IMOD 
ILAW 
F 
7 
BC 
F 
7 
F 
8 
8 
5 
BT 
F 
5 
6 
AC 
F 
6 
Variable 
SFSTI 
SFSTR 
CRIN 
ECRCL 
NCYCR 
NIPF 
Type 
F 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
RO 
E 
PR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Mass density 𝜌. 
Young’s modulus 𝐸. 
Poisson’s ratio 𝜈.
IMOD 
*MAT_280 
DESCRIPTION
Flag  to  choose  degradation  procedure,  when  critical  stress  is
reached. 
EQ.0.0: Softening in NCYCR load steps.  Define SFSTI, SFSTR,
and NCYCR (default). 
EQ.1.0: Damage  model  for  softening.    Define  ILAW,  AT,  BT,
AC, and BC. 
ILAW 
Flag to choose damage evolution law if IMOD = 1.0, see Remarks.
EQ.0.0: Same  damage  evolution  for  tensile  and  compressive 
failure (default). 
EQ.1.0: Different  damage  evolution  for  tensile  failure  and
compressive failure. 
FMOD 
Flag to choose between failure criteria, see Remarks. 
EQ.0.0: Rankine maximum stress (default), 
EQ.1.0: Mohr-Coulomb,  
EQ.2.0: Drucker-Prager. 
Tensile strength 𝑓𝑡. 
Compressive strength 𝑓𝑐. 
Tensile damage evolution parameter 𝛼𝑡.  Can be interpreted as the 
residual  load  carrying  capacity  ratio  for  tensile  failure  ranging
from 0 to 1. 
Tensile damage evolution parameter 𝛽𝑡.  It controls the softening 
velocity for tensile failure. 
Compressive damage evolution parameter 𝛼𝑡.  Can be interpreted 
as the residual load carrying capacity ratio for compressive failure
ranging from 0 to 1. 
Compressive  damage  evolution  parameter  𝛽𝑡.    It  controls  the 
softening velocity for compressive failure. 
Scale factor for stiffness after failure, e.g. SFSTI = 0.001 means that 
stiffness is reduced to 0.1% of the elastic stiffness at failure. 
Scale  factor  for  stress  in  case  of  failure,  e.g.  SFSTR = 0.01  means 
that stress is reduced to 1% of the failure stress at failure. 
FT 
FC 
AT 
BT 
AC 
BC 
SFSTI 
SFSTR
*MAT_GLASS 
DESCRIPTION
ICRIN 
Flag for crack strain initialization 
EQ.0.0: initial crack strain is strain at failure (default), 
EQ.1.0: initial crack strain is zero. 
Crack  strain  necessary  to  reactivate  certain  stress  components
after crack closure.  
Number of cycles in which the stress is reduced to SFSTR*failure
stress. 
Number  of  failed  through  thickness  integration  points  to  fail  all
through thickness integration points for IMOD = 0. 
ECRCL 
NCYCR 
NIPF 
Remarks: 
The underlying material behavior before failure is isotropic, small strain linear elasticity 
with  Young’s  modulus  𝐸  and  Poisson’s  ratio  𝜈.    Asymmetric  (tension-compression 
dependent) failure happens as soon as one of the following plane stress failure criteria is 
violated. 
For FMOD = 0, a maximum stress  criterion (Rankine) is used, where principal stresses 
𝜎1 and 𝜎2 are bound by tensile strength 𝑓𝑡 and compressive strength 𝑓𝑐 as follows: 
−𝑓𝑐 < {𝜎1, 𝜎2} < 𝑓𝑡 
With  FMOD = 1,  the  Mohr-Coulomb  criterion  with  expressions  in  four  different 
categories is used: 
𝜎1 > 0 and 𝜎2 > 0:   max (
𝜎1 < 0 and 𝜎2 < 0:   max (−
𝜎1
𝑓𝑡
𝜎1
𝑓𝑐
,
𝜎2
𝑓𝑡
) < 1 
, −
𝜎2
𝑓𝑐
) < 1 
𝜎1 > 0 and 𝜎2 < 0:  
−
< 1 
𝜎1 < 0 and 𝜎2 > 0:  −
+
< 1 
𝜎1
𝑓𝑡
𝜎1
𝑓𝑐
𝜎2
𝑓𝑐
𝜎2
𝑓𝑡
And for FMOD = 2, the plane stress Drucker-Prager criterion is given by 
2𝑓𝑐
[(
𝑓𝑐
𝑓𝑡
− 1) (𝜎1 + 𝜎2) + (
𝑓𝑐
𝑓𝑡
+ 1) √𝜎1
2 + 𝜎2
2 − 𝜎1𝜎2] < 1
As  soon  as  failure  happens  in  the  tensile  regime,  a  crack  occurs  perpendicular  to  the 
maximum  principal  stress  direction.    That  means  a  crack  coordinate  system  is  set  up 
and  stored,  defined  by  a  relative  angle  with respect  to  the  element  coordinate  system.  
Appropriate  stress  and  stiffness  tensor  components  (e.g.    normal  to  the  crack)  are 
reduced according to SFSTR and SFSTI if IMOD = 0.  The stress reduction takes place in 
a period of NCYCR time step cycles. For IMOD = 1.0 the stress and stiffness tensor are 
reduced by a damage model, please see below.  A second crack orthogonal to the first 
crack  is  possible  which  can  open  and  close  independently  from  the  first  one,  further 
reducing the element stiffness. 
To  deal  with  crack  closure,  the  current  strain  in  principal  stress  direction  is  stored  as 
initial  crack  strain  (ICRIN = 0,  default)  or  the  initial  crack  strain  is  set  to  zero 
(ICRIN = 1).  After failure, the crack strain is tracked, so that later crack closure will be 
detected.    If  that  is  the  case,  appropriate  stress  and  stiffness  tensor  components  (e.g.  
compressive)  are  reactivated  so  that  e.g.    under  pressure  a  load  could  be  carried  and 
cause a nonzero stress perpendicular to the crack. 
If  the  critical  number  of  failed  integration  points  (NIPF)  in  one  element  is  reached,  all 
integration points over the element thickness fail as well.  The default value of NIPF = 1 
resembles the fact, that a crack in a glass plate immediately runs through the thickness. 
Starting  with  the  Release  of  LS-DYNA  version  R10,  a  damage  model  for  stress  and 
stiffness  softening  can  be  activated  with  IMOD = 1.    The  corresponding  evolution  law 
for ILAW = 0 is given by 
𝐷 =
{⎧
{⎨
⎩
1 −
0                                                    𝑓𝑜𝑟 𝜅 ≤ 𝜅0
𝜅0
(1 − 𝛼𝑡,𝑐 + 𝛼𝑡,𝑐𝑒−𝛽𝑡,𝑐 (𝜅−𝜅0))      𝑒𝑙𝑠𝑒                   
i.e.  tensile and compressive failure are treated in the same fashion.  
On the other hand, with ILAW = 1, the damage evolution for tensile failure is given by 
𝐷 =
{⎧
{⎨
⎩
0                                                    𝑓𝑜𝑟 𝜅 ≤ 𝜅0
𝜅0
(1 − 𝛼𝑡 + 𝛼𝑡𝑒−𝛽𝑡 (𝜅−𝜅0))      𝑒𝑙𝑠𝑒                   
1 −
whereas  damage  for  compressive  failure  evolves  like  that  (more  delayed  stress 
reduction): 
𝐷 =
{⎧
{⎨
⎩
0                                                    𝑓𝑜𝑟 𝜅 ≤ 𝜅0
𝜅0
(1 − 𝛼𝑐) − 𝛼𝑐𝑒−𝛽𝑐 (𝜅−𝜅0)      𝑒𝑙𝑠𝑒                   
1 −
*MAT_GLASS 
  VARIABLE   
DESCRIPTION
1 
2 
3 
Crack flag:  
0 = no  crack,  1 = one  crack,  2 = two  cracks,  -1 = failed  under 
compression 
Direction of 1st principle stress as angle in radiant with respect to
the element direction.  The shell normal defines the positive angle
direction.  The 1st crack direction is perpendicular to the direction
of 1st principle stress. 
Angle  in  radiant  that  defines  the  orthogonal  to  the  2nd  crack 
direction (with respect to the element direction).
*MAT_293 
This  is  Material  Type  293.    This  material  models  the  behavior  of  pre-impregnated 
(prepreg)  composite  fibers  during  the  high  temperature  preforming  process.    In 
addition to providing stress and strain, it also provides warp and weft yarn directions 
and stretch ratios after the forming process.  The major applications of the model are for 
materials used in light weight automobile parts. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
  Card 2 
1 
2 
RO 
F 
2 
3 
ET 
F 
3 
4 
EC 
F 
4 
Variable 
G124 
G125 
G126 
GAMMAL
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
F 
4 
Variable 
VM 
EPSILON 
THETA 
BULK 
Type 
F 
F 
F 
F 
5 
PR 
F 
5 
VF 
F 
5 
G 
F 
  VARIABLE   
DESCRIPTION
6 
7 
8 
G121 
G122 
G123 
F 
6 
F 
7 
F 
8 
EF3 
VF23 
EM 
F 
6 
F 
7 
F 
8 
MID 
RO 
ET 
EC 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Continuum equivalent mass density. 
Tensile modulus along the fiber yarns, corresponding to the slope
of the curve in Figure M293-2 in the Stable Modulus region from a 
uniaxial tension test.  See Remark 5. 
Compression  modulus  along  the  fiber  yarns,  reversely  calculated
using  bending  tests  when  all  the  other  material  properties  are
determined.  See Remark 5.
VARIABLE   
DESCRIPTION
PR 
G12i 
Poisson’s ratio.  See Remark 5. 
Coefficients for the bias-extension angle change-engineering stress 
curve in Figure M293-3.  G121 to G126 corresponds to the 6th order 
to 1st order factors of the loading curve.  See Remark 5. 
GAMMAL 
Shear locking angle, in degrees.  See Remark 5. 
VF 
EF3 
Fiber volume fraction in the prepreg composite. 
Transverse compression modulus of the dry fiber. 
VF23 
Transverse Poisson’s ratio of the dry fiber 
EM 
VM 
EPSILON 
THETA 
Young’s modulus of the cured resin. 
Poisson’s ratio of the cured resin 
Stretch  ratio  at  the  end  of  undulation  stage  during  the  uniaxial
tension test.  Example shown in Figure M293-2.  See Remark 5. 
Initial  angle  offset  between  the  fiber  direction  and  the  element
direction.    To  reduce  simulation  error,  when  building  the  model,
the  elements  should  be  aligned  to  the  same  direction  as  much  as
possible. 
BULK 
Bulk modulus of the prepreg material 
G 
Shear modulus of the prepreg material 
Remarks: 
1.  Fiber and Resin Properties.  The dry fiber properties, EF3 and VF23, and the 
cure resin properties, EM and VM, are used to calculate the through thickness 
elastic modulus of the prepreg using the rule of mixture.  These properties will 
not  affect  the  in-plane  deformation  of  the  prepreg  during  the  preforming 
simulation. 
2.  Shear  Locking.    In  most  of  the  preforming  cases,  the  angle  between  the  fiber 
yarns  will  not  reach  the  shear  locking  state.    This  model  is  not  designed  for, 
and, therefore, not recommended for simulating shear locking.
3.  BULK and G.  BULK and G are used by the contact algorithm.  Changing these 
parameters  will  not  affect  the  final  simulation  result  significantly  (but  it  may 
affect the time step). 
4.  Model Description.  Woven composite prepregs are characterized using a non-
orthogonal coordinate system having two principal directions: one aligned with 
the longitudinal warp yarns and the other with the transverse weft yarns.  Prior 
to deformation the warp and weft yarns are orthogonal.  The directions and the 
fiber  stretch  ratios  are  determined  from  the  deformation  gradient.    In  Figure 
M293-1, the angles 𝛼 and 𝛽 refer to the relative of the rotation of the warp yarn 
coordinate  to  the  local  corotational  𝑥  coordinate  and  the  angle  between  the 
warp and weft yarns, respectively [2,3,4].   
The stress from material deformation is divided into two parts: (1) stress caused 
by the fiber stretch, 𝛔𝑓 , as shown in Figure M293-1 (a); (2) stress caused by the 
fiber rotation, 𝛔𝑚, as shown in Figure M293-1 (b).  The total stress tensor, 𝛔, in 
the local corotational 𝑥 − 𝑦 coordinate system is the sum where the components 
are given below [3]: 
𝑓 = 𝜎𝑦𝑥
𝜎𝑥𝑦
𝜎𝑥𝑦
𝑚 = 𝜎𝑦𝑥
𝑓 sin 2(𝛼 + 𝛽) #(2)
𝜎2
𝑓 = 𝜎1
𝑓 cos2(𝛼 + 𝛽) #(1)
𝑓 cos2 𝛼 +   𝜎2
𝜎𝑥𝑥
𝑓 =
𝑓 sin 2𝛼 +
𝜎1
𝑓 = 𝜎1
𝑓 sin2(𝛼 + 𝛽) #(3)
𝑓 sin2 𝛼 + 𝜎2
𝜎𝑦𝑦
𝑚 − 𝜎2
𝑚 + 𝜎2
𝜎1
𝜎1
𝑚 − 𝜎2
𝜎1
𝑚 + 𝜎2
𝜎1
𝑓 + 𝜎𝑥𝑥
sin(2𝛼 + 𝛽) #(5)
𝑚 − 𝜎2
𝜎1
𝜎𝑥𝑥 = 𝜎𝑥𝑥
𝑚 #(7)
𝑚 =
𝑚 =
𝑚 =
𝜎𝑦𝑦
𝜎𝑥𝑥
−
+
cos(2𝛼 + 𝛽) #(4)
cos(2𝛼 + 𝛽) #(6)
𝜎𝑥𝑦 = 𝜎𝑦𝑥 = 𝜎𝑥𝑦
𝑓 + 𝜎𝑥𝑦
𝑚 #(8)
𝜎𝑦𝑦 = 𝜎𝑦𝑦
𝑓 + 𝜎𝑦𝑦
𝑚 #(9)
5.  Material  Property  Characterization.    The  non-orthogonal  stress  components 
caused by yarn stretch and rotation at various deformation states will be char-
acterized  via  a  set  of  experiments,  which  are  uniaxial  tension,  bias-extension 
and  cantilever  beam  bending  tests.    All  the  tests  need  to  be  performed  at  the 
preforming temperature.  See references [1] and [3] for more details.
𝑦 
𝑓  
𝜎2
𝑚 
𝜎2
𝜎1
𝛽 
𝛼 
(a) 
𝑚 
𝜎1
(b
) 
Figure  M293-1.    Stress  components  caused  by  (a)  stretch  in  fiber  directions
and (b) rotation of the fibers [3]. 
400
350
300
250
200
150
100
50
)
(
Undulation
region
Stable Modulus
region
0.00% 1.00% 2.00% 3.00% 4.00% 5.00%
Stretch Ratio
Figure M293-2.  An example of the engineering stress as a function of stretch
ratio from the uniaxial tension test [3]. 
The uniaxial tension test is used to obtain the fiber direction undulation strains 
and the stable tensile moduli, together with the in-plane Poisson’s ratio (PR).  A 
typical  test  result  is  shown  in  Figure  M293-2.    From  the  stretch  ratio-
engineering  stress  curve,  the  tensile  modulus,  ET,  and  the  stretch  ratio  at  the 
end of undulation, EPSILON, can be captured. 
The bias-extension test is used to characterize the shear behavior of the compo-
site needed for fields G12𝑖.  The test procedure comes from the benchmark test 
literature  [1].    An  example  of  the  bias-extension  test  angle  change-engineering 
stress curve is shown in Figure M293-3.
)
(
0.1
0.08
0.06
0.04
0.02
Curve fitting
0.2
0.4
1.0
Angle change (radians)
0.6
0.8
1.2
1.4
Figure  M293-3.    An  example  of  the  angle  change-engineering  stress  curve
from  the  bias-extension  test.    The  curve  fit  for  this  example  is  𝑦 = −0.29𝑥6 +
1.09𝑥5 − 1.68𝑥4 + 1.37𝑥3 − 0.56𝑥2 + 0.12𝑥 .    For  this  example  curve  the  inputs
into  LS-DYNA  are  G121 = −0.29,  G122 = 1.09,  G123 = −1.68,  G124 = 1.37,
G125 = −0.56, and G126 = −0.12 [3]. 
Thermometer
Forming Temp
Ruler
Composite
Support & 
Clamp
Heating Chamber
Figure M293-4.  Bending test setup [3] 
The angle change is calculated by using the equation [1]: 
𝛾 =
− 2 cos−1 𝐷 + 𝑑
√2𝐷
where  𝑑  is  the  cross-head  displacement  and  𝐷  is  the  difference  between  the 
original height and the original width of the sample.  This equation holds only 
before the shear locking angle, specified in field GAMMAL, which is measured 
directly at the end of the test, so the curve should end when the fiber yarn angle 
reaches the shear locking state. 
The bending test should be performed to characterize the compression modulus 
along the yarn directions, as specified in the EC field.  The test setup is shown 
in  Figure  M293-4.    The  composite  specimen  is  held  in  a  clamp  and  deforms 
under its own gravity.  During the test, the composite is heated to the preform-
ing temperature and the tip displacement is recorded.  Due to the nonlinearity 
of the tensile modulus, the compression modulus is reversely calculated using a 
simulation: it is adjusted until the simulation leads to similar tip displacement
to  the  real  experiment  case.    The  starting  point  for  the  compression  modulus 
iteration can be set as about 100X of the shear modulus when the warp and weft 
yarns are perpendicular to each other. 
6.  Element Type.  The material model is available for shell elements with OSU=1 
and  INN=2  in  the  CONTROL_ACCURACY  card.    It  is  recommended  to  use  a 
double precision version of LS-DYNA. 
References: 
 [1]   J.  Cao, R.  Akkerman, P.  Boisse, J.  Chen, H.S.  Cheng, E.F.  de Graaf, J.L.  
Gorczyca, P.  Harrison, G.  Hivet, J.  Launay, W.  Lee, L.  Liu, S.V.  Lomov, A.  
Long, E.  de Luycker, F.  Morestin, J.  Padvoiskis, X.Q.  Peng, J.  Sherwood, Tz.  
Stoilova, X.M.  Tao, I.  Verpoest, A.  Willems, J.  Wiggers, T.X.  Yu, B.  Zhu, 
Characterization of mechanical behavior of woven fabrics: Experimental methods 
and benchmark results, Composites Part A: Applied Science and Manufacturing, 
Volume 39, Issue 6, 2008, Pages 1037-1053, ISSN 1359-835X. 
 [2]   Pu Xue, Xiongqi Peng, Jian Cao, A non-orthogonal constitutive model for 
characterizing woven composites, Composites Part A: Applied Science and 
Manufacturing, Volume 34, Issue 2, 2003, Pages 183-193, ISSN 1359-835X. 
 [3]   Weizhao Zhang, Huaqing Ren, Biao Liang, Danielle Zeng, Xuming Su, Jeffrey 
Dahl, Mansour Mirdamadi, Qiangsheng Zhao, Jian Cao, A non-orthogonal 
material model of woven composites in the preforming process, CIRP Annals - 
Manufacturing Technology, Volume 66, Issue 1, 2017, Pages 257-260, ISSN 0007-
8506. 
 [4]   X.Q.  Peng, J.  Cao, A continuum mechanics-based non-orthogonal constitutive 
model for woven composite fabrics, Composites Part A: Applied Science and 
Manufacturing, Volume 36, Issue 6, 2005, Pages 859-874, ISSN 1359-835X.
See *MAT_VACUUM or *MAT_140.
*MAT_ALE_01
*MAT_ALE_GAS_MIXTURE 
This  may  also  be  referred  to  as  *MAT_ALE_02.    This  model  is  used  to  simulate 
thermally equilibrated ideal gas mixtures.  This only works with the multi-material ALE 
formulation  (ELFORM = 11  in  *SECTION_SOLID).    This  keyword  needs  to  be  used 
together  with  *INITIAL_GAS_MIXTURE  for  the  initialization  of  gas  densities  and 
temperatures.    When  applied  in  the  context  of  ALE  airbag  modeling,  the  injection  of 
inflator  gas  is  done  with  a  *SECTION_POINT_SOURCE_MIXTURE  command  which 
controls the injection process.  This is an identical material model to the *MAT_GAS_-
MIXTURE model. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
IADIAB 
RUNIV 
Type 
A8 
Default 
none 
Remark 
I 
0 
5 
F 
0.0 
1 
Card 2 for Per mass Calculation.  Method (A) RUNIV = blank or 0.0. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  CVmass1  CVmass2  CVmass3 CVmass4 CVmass5 CVmass6  CVmass7  Cvmass8
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none
Card 3 for Per mass Calculation.  Method (A) RUNIV = blank or 0.0. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  CPmass1  CPmass2  CPmass3 CPmass4 CPmass5 CPmass6  CPmass7  Cpmass8
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Card 2 for Per Mole Cclculation.  Method (B) RUNIV is nonzero. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MOLWT1  MOLWT2  MOLWT3 MOLWT4 MOLWT5 MOLWT6  MOLWT7  MOLWT8
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Remark 
2 
Card 3 for Per Mole Cclculation.  Method (B) RUNIV is nonzero. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CPmole1  CPmole2  CPmole3  CPmole4  CPmole5  CPmole6  Cpmole7  CPmole8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Remark
Card 4 for Per Mole Cclculation.  Method (B) RUNIV is nonzero. 
  Card 4 
Variable 
1 
B1 
Type 
F 
2 
B2 
F 
3 
B3 
F 
4 
B4 
F 
5 
B5 
F 
6 
B6 
F 
7 
B7 
F 
8 
B8 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Remark 
2 
Card 5 for Per Mole Cclculation.  Method (B) RUNIV is nonzero. 
  Card 5 
Variable 
1 
C1 
Type 
F 
2 
C2 
F 
3 
C3 
F 
4 
C4 
F 
5 
C5 
F 
6 
C6 
F 
7 
C7 
F 
8 
C8 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Remark 
2 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
IADIAB 
This  flag  (default = 0)  is  used  to  turn  ON/OFF  adiabatic 
compression logics for an ideal gas (remark 5). 
EQ.0: OFF (default) 
EQ.1: ON 
RUNIV 
Universal gas constant in per-mole unit (8.31447 J/(mole*K)). 
CVmass1 - 
CVmass8 
If  RUNIV  is  BLANK  or  zero  (method  A):  Heat  capacity  at
constant volume for up to eight different gases in per-mass unit.
VARIABLE   
DESCRIPTION
CPmass1 - 
CPmass8 
If  RUNIV  is  BLANK  or  zero  (method  A):  Heat  capacity  at 
constant pressure for up to eight different gases in per-mass unit.
MOLWT1 - 
MOLWT8 
If RUNIV is nonzero (method B):  Molecular weight of each ideal
gas in the mixture (mass-unit/mole). 
If  RUNIV  is  nonzero  (method  B):  Heat  capacity  at  constant 
pressure  for  up  to  eight  different  gases  in  per-mole  unit.    These 
are  nominal  heat  capacity  values  typically  at  STP.    These  are
denoted by the variable “A” in the equation in remark 2. 
If  RUNIV  is  nonzero  (method  B):  First  order  coefficient  for  a 
temperature dependent heat capacity at constant pressure for up
to eight different gases.  These are denoted by the variable “B” in
the equation in remark 2. 
If  RUNIV  is  nonzero  (method  B):  Second  order  coefficient  for  a 
temperature dependent heat capacity at constant pressure for up
to eight different gases.  These are denoted by the variable “C” in
the equation in remark 2. 
CPmole1 - 
CPmole8 
B1 - B8 
C1 - C8 
Remarks: 
1.  There are 2 methods of defining the gas properties for the mixture.  If RUNIV is 
BLANK  or  ZERO  →  Method  (A)  is  used  to  define  constant  heat  capacities 
where  per-mass  unit  values  of  Cv  and  Cp  are  input.    Only  cards  2  and  3  are 
required for this method.  Method (B) is used to define constant or temperature 
dependent heat capacities where per-mole unit values of Cp are input.  Cards 2-
5 are required for this method. 
2.  The per-mass-unit, temperature-dependent, constant-pressure heat capacity is 
𝐶𝑝(𝑇) =
(CPMOLE + B × 𝑇 + C × 𝑇2)
MOLWT
Typical metric units: 
𝐶𝑝(𝑇) 
kg 𝐾
CPMOLE
A 
mole K
mole K2
mole K3
3.  The initial temperature and the density of the gas species present in a mesh or 
part at time zero is specified by the keyword *INITIAL_GAS_MIXTURE. 
4.  The ideal gas mixture is assumed to be thermal equilibrium, that is, all species 
are at the same temperature (T).  The gases in the mixture are also assumed to 
follow Dalton’s Partial Pressure Law, 
ngas
𝑃 = ∑ 𝑃𝑖
. 
The partial pressure of each gas is then 
𝑃𝑖 = 𝜌𝑖𝑅gas𝑖
𝑇 
Where 
𝑅gas𝑖
=
𝑅univ
MOLWT
. 
The  individual  gas  species  temperature  equals  the  mixture  temperature.    The 
temperature  is  computed  from  the  internal  energy  where  the  mixture  internal 
energy per unit volume is used, 
whence 
𝑇 = 𝑇𝑖 =
𝑒𝑉
ngas
∑ 𝜌𝑖𝐶𝑉𝑖
ngas
𝑒𝑉 = ∑ 𝜌𝑖𝐶𝑉𝑖
ngas
𝑇𝑖 
= ∑ 𝜌𝑖𝐶𝑉𝑖
𝑇. 
In  general,  the  advection  step  conserves  momentum  and  internal  energy,  but 
not  kinetic  energy.    This  can  result  in  energy  lost  in  the  system  and  lead  to  a 
pressure  drop.    In  *MAT_GAS_MIXTURE  the  dissipated  kinetic  energy  is  au-
tomatically stored in the internal energy.  Thus in effect the total energy is con-
served  instead  of  conserving  just  the  internal  energy.    This  numerical  scheme 
has been shown to improve accuracy in some cases.  However, the user should 
always be vigilant and check the physics of the problem closely. 
5.  As an example  consider an airbag surrounded by ambient air.  As the inflator 
gas flows into the bag, the ALE elements cut by the airbag fabric shell elements 
will contain some inflator gas inside and some ambient air outside.  The multi-
material element treatment is not perfect.  Consequently the temperature of the 
outside air may, occasionally, be made artificially high after the multi-material 
element treatment.  To prevent the outside ambient air from getting artificially 
high T, set IDIAB = 1 for the ambient air outside.  Simple adiabatic compression 
equation is then assumed for the outside air.  The use of this flag may be need-
ed,  but  only  when  that  outside  air  is  modeled  by  the  *MAT_GAS_MIXTURE 
card. 
Example: 
Consider  a  tank  test  model  where  the  Lagrangian  tank  (Part  S1)  is  surrounded  by  an 
ALE  air  mesh  (Part  H4 = AMMGID  1).    There  are  2  ALE  parts  which  are  defined  but 
initially  have  no  corresponding  mesh:  part  5  (H5 = AMMGID  2)  is  the  resident  gas 
inside  the  tank  at  t = 0,  and  part  6  (H6 = AMMGID  2)  is  the  inflator  gas(es)  which  is 
injected into the tank when t > 0.  AMMGID stands for ALE Multi-Material Group ID.  
Please see figure and input below.  The *MAT_GAS_MIXTURE (MGM) card defines the 
gas properties of ALE parts H5 & H6.  The MGM card input for both method (A) and 
(B) are shown. 
The  *INITIAL_GAS_MIXTURE  card  is  also  shown.    It  basically  specifies  that  “AM-
MGID 2 may be present in part or mesh H4 at t = 0, and the initial density of this gas is 
defined in the rho1 position which corresponds to the 1st material in the mixture (or H5, 
the resident gas).” 
Example configuration: 
Cut-off view
S1 = tank  
H4 = AMMG1 = backgrou
nd  outside  air  (initially 
defined ALE mesh) 
H5 = AMMG2 = initial 
gas 
inside  the  tank  (this  has  no 
initial mesh)
H6 = AMMG2 = inflator 
gas(es) injected in (this has no 
initial mesh)
Sample input: 
$------------------------------------------------------------------------------- 
*PART 
H5 = initial gas inside the tank 
$      PID     SECID       MID     EOSID      HGID      GRAV    ADPOPT      TMID 
         5         5         5         0         5         0         0 
*SECTION_SOLID 
         5        11         0 
$------------------------------------------------------------------------------- 
$ Example 1:  Constant heat capacities using per-mass unit. 
$*MAT_GAS_MIXTURE
$      MID    IADIAB    R_univ 
$        5         0         0  
$  Cv1_mas   Cv2_mas   Cv3_mas   Cv4_mas   Cv5_mas   Cv6_mas   Cv7_mas   Cv8_mas 
$718.7828911237.56228 
$  Cp1_mas   Cp2_mas   Cp3_mas   Cp4_mas   Cp5_mas   Cp6_mas   Cp7_mas   Cp8_mas 
$1007.00058 1606.1117 
$------------------------------------------------------------------------------- 
$ Example 2:  Variable heat capacities using per-mole unit. 
*MAT_GAS_MIXTURE 
$      MID    IADIAB    R_univ 
         5         0  8.314470 
$      MW1       MW2       MW3       MW4       MW5       MW6       MW7       MW8 
 0.0288479   0.02256 
$  Cp1_mol   Cp2_mol   Cp3_mol   Cp4_mol   Cp5_mol   Cp6_mol   Cp7_mol   Cp8_mol 
 29.049852  36.23388 
$       B1        B2        B3        B4        B5        B6        B7        B8 
  7.056E-3  0.132E-1 
$       C1        C2        C3        C4        C5        C6        C7        C8 
 -1.225E-6 -0.190E-5 
$------------------------------------------------------------------------------- 
$ One card is defined for each AMMG that will occupy some elements of a mesh set 
*INITIAL_GAS_MIXTURE 
$      SID     STYPE     MMGID        T0 
         4         1         1    298.15 
$     RHO1      RHO2      RHO3      RHO4      RHO5      RHO6      RHO7      RHO8 
1.17913E-9 
*INITIAL_GAS_MIXTURE 
$      SID     STYPE     MMGID        T0 
         4         1         2    298.15 
$     RHO1      RHO2      RHO3      RHO4      RHO5      RHO6      RHO7      RHO8 
1.17913E-9 
$-------------------------------------------------------------------------------
F 
0.0 
*MAT_ALE_VISCOUS 
*MAT_ALE_VISCOUS 
*MAT_ALE_03 
This may also be referred to as MAT_ALE_03.  This “fluid-like” material model is very 
similar to Material Type 9 (*MAT_NULL).  It allows the modeling of non-viscous fluids 
with constant or variable viscosity.  The variable viscosity is a function of an equivalent 
deviatoric strain rate.  If inviscid material is modeled, the deviatoric or viscous stresses 
are  zero,  and  the  equation  of  state  supplies  the  pressures  (or  diagonal  components  of 
the stress tensor).  All *MAT_ALE_cards apply only to ALE element formulation. 
  Card 1 
1 
Variable 
MID 
Type 
I 
2 
RO 
F 
3 
PC 
F 
4 
5 
6 
7 
8 
MULO 
MUHI 
RK 
Not used 
RN 
F 
F 
F 
Defaults 
none 
none 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
MID 
Material identification.  A unique number has to be chosen. 
RO 
PC 
Mass density. 
Pressure cutoff (≤ 0.0).  See Remark 4. 
MULO 
There are 4 possible cases : 
1. 
2. 
3. 
4. 
If MULO = 0.0, then inviscid fluid is assumed. 
If  MULO > 0.0,  and  MUHI = 0.0  or  is  not  defined,  then 
this  is  the  traditional  constant  dynamic  viscosity  coeffi-
cient 𝜇. 
If MULO > 0.0, and MUHI > 0.0, then MULO and MUHI 
are  lower  and  upper  viscosity  limit  values  for  a  power-
law-like variable viscosity model. 
If  MULO  is  negative  (for  example,  MULO = -1),  then  a 
user-input  data  load  curve  (with  LCID = 1)  defining  dy-
namic  viscosity  as  a  function  of  equivalent  strain  rate  is
used.
VARIABLE   
DESCRIPTION
MUHI 
There are 2 possible cases: 
5. 
6. 
in 
If  MUHI < 0.0,  then  the  viscosity  can  be  defined  by  the
file  dyn21.F  with  a  routine  called 
user 
f3dm9ale_userdef1.    The  file  is  part  of  the  general  us-
ermat package.  
the 
If  MUHI > 0.0,  then  this  is  the  upper  dynamic  viscosity
limit  (default = 0.0).    This  is  defined  only  if  RK  and  RN 
are defined for the variable viscosity case. 
Variable dynamic viscosity multiplier.  See Remark 6. 
Variable dynamic viscosity exponent.  See Remark 6. 
RK 
RN 
Remarks: 
1.  Deviatoric Viscous Stress.  The null material must be used with an equation-
of-state.  Pressure cutoff is negative in tension.  A (deviatoric) viscous stress of 
the form 
𝜎𝑖𝑗
′  
′ = 2𝜇𝜀̇𝑖𝑗
[
𝑚2] ~ [
𝑚2 𝑠] [
] 
is  computed  for  nonzero  𝜇  where  𝜀̇𝑖𝑗
namic viscosity.  For example, in SI unit system, 𝜇 has a unit of [Pa × s]. 
′   is  the  deviatoric  strain  rate.   𝜇  is  the  dy-
2.  Hourglass  Control  Issues.    The  null  material  has  no  shear  stiffness  and 
hourglass  control  must  be  used  with  care.    In  some  applications,  the  default 
hourglass  coefficient  might  lead  to  significant  energy  losses.    In  general  for 
fluid(s), the hourglass coefficient QM should be small (in the range 10−4 to 10−6 
for the standard default IHQ choice). 
3.  Null Material Properties.  Null material has no yield strength and behaves in a 
fluid-like manner. 
4.  Numerical Cavitation.  The pressure cut-off, PC, must be defined to allow for a 
material to “numerically” cavitate.  In other words, when a material undergoes 
dilatation  above  certain  magnitude,  it  should  no  longer  be  able  to  resist  this 
dilatation.    Since  dilatation  stress  or  pressure  is  negative,  setting  PC  limit  to  a 
very  small  negative  number  would  allow  for  the  material  to  cavitate  once  the 
pressure in the material goes below this negative value.
5. 
Issues with Small Values of Viscosity Exponent.  If the viscosity exponent is 
less than 1.0, RN < 1.0, then RN − 1.0 < 0.0.  In this case, at very low equivalent 
strain rate, the viscosity can be artificially very high.  MULO is then used as the 
viscosity value. 
6.  Empirical  Dynamic  Viscosity.    The  empirical  variable  dynamic  viscosity  is 
typically  modeled  as  a  function  of  equivalent  shear  rate  based  on  experimental 
data. 
For an incompressible fluid, this may be written equivalently as 
μ(𝛾̅̅̅̅̇ ′) = RK × 𝛾̅̅̅̅̇ ′(𝑅𝑁−1)
μ(𝜀̅
̇′) = RK × 𝜀̅
̇′(𝑅𝑁−1)
The “overbar” denotes a scalar equivalence.  The “dot” denotes a time deriva-
tive or rate effect.  And the “prime” symbol denotes deviatoric or volume pre-
serving components.  The equivalent shear rate components may be related to the 
basic definition of (small-strain) strain rate components as follows: 
𝜀̇𝑖𝑗 =
(
∂𝑢𝑖
∂𝑥𝑗
+
∂𝑢𝑗
∂𝑥𝑖
𝛾̇𝑖𝑗 = 2𝜀̇𝑖𝑗 
) ⇒ 𝜀̇𝑖𝑗
′ = 𝜀̇𝑖𝑗 − 𝛿𝑖𝑗 (
𝜀̇𝑘𝑘
) 
Typically, the 2nd invariant of the deviatoric strain rate tensor is defined as: 
The equivalent (small-strain) deviatoric strain rate is defined as:  
𝐼2𝜀̅
̇′ =
[𝜀̇𝑖𝑗
′ 𝜀̇𝑖𝑗
′ ] 
𝜀̅′̇ ≡ 2√𝐼2𝜀′̇ = √2[𝜀̇𝑖𝑗
′ 𝜀̇𝑖𝑗
′ ] = √4[𝜀̇12
′ 2 + 𝜀̇23
′ 2 + 𝜀̇31
′ 2] + 2[𝜀̇11
′ 2 + 𝜀̇22
′ 2 + 𝜀̇33
′ 2] 
In non-Newtonian literatures, the equivalent shear rate is sometimes defined as  
𝛾̅̅̅̅̇ ≡ √
𝛾̇𝑖𝑗𝛾̇𝑖𝑗
= √2𝜀̇𝑖𝑗𝜀̇𝑖𝑗 = √4[𝜀̇12
2 + 𝜀̇23
2 + 𝜀̇31
2 ] + 2[𝜀̇11
2 + 𝜀̇22
2 + 𝜀̇33
2 ] 
It  turns  out  that,  (a)  for  incompressible  materials  (𝜀̇𝑘𝑘 = 0),  and  (b)  the  shear 
′ , the equivalent shear rate is algebraical-
terms are equivalent when 𝑖 ≠ 𝑗→ 𝜀̇𝑖𝑗 = 𝜀̇𝑖𝑗
ly equivalent to the equivalent (small-strain) deviatoric strain rate. 
̇′ = 𝛾̅̅̅̅̇ ′
𝜀̅
*MAT_ALE_MIXING_LENGTH 
This may also be referred to as *MAT_ALE_04.  This viscous “fluid-like” material model 
is  an  advanced  form  of  *MAT_ALE_VISCOUS.    It  allows  the  modeling  of  fluid  with 
constant  or  variable  viscosity  and  a  one-parameter  mixing-length  turbulence  model.  
The variable viscosity is a function of an equivalent deviatoric strain rate.  The equation 
of state supplies the pressures for the stress tensor.  All *MAT_ALE_cards apply only to 
ALE element formulation.  
Card Format 
  Card 1 
1 
Variable 
MID 
Type 
I 
2 
RO 
F 
3 
PC 
F 
4 
5 
6 
7 
8 
MULO 
MUHI 
RK 
Not used 
RN 
F 
F 
F 
Defaults 
none 
0.0 
0.0 
0.0 
0.0 
0.0 
Internal Flow Card. 
  Card 2 
Variable 
1 
LC 
Type 
F 
2 
C0 
F 
3 
C1 
F 
4 
C2 
F 
5 
C3 
F 
6 
C4 
F 
7 
C5 
F 
F 
0.0 
8 
C6 
F 
Defaults 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
External Flow Card. 
  Card 3 
Variable 
1 
LC 
Type 
F 
2 
D0 
F 
3 
D1 
F 
4 
D2 
F 
5 
E0 
F 
6 
E1 
F 
7 
E2 
F 
8 
Defaults 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0
VARIABLE   
DESCRIPTION
MID 
Material identification.  A unique number has to be chosen. 
Mass density 
Pressure cutoff (≤ 0.0). 
There are 3 possible cases:  (1) If MULO > 0.0, and MUHI = 0.0 or 
is  not  defined,  then  this  is  the  traditional  constant  dynamic
viscosity  coefficientμ.    (2)  If  MULO > 0.0,  and  MUHI > 0.0,  then 
MULO and MUHI are lower and upper viscosity limit values.  (3) 
If MULO is negative (for example, MULO = -1), then a user-input 
data  load  curve  (with  LCID = 1)  defining  dynamic  viscosity  as  a 
function of equivalent strain rate is used. 
Upper  dynamic  viscosity  limit  (default = 0.0).    This  is  defined 
only if RK and RN are defined for the variable viscosity case. 
Variable dynamic viscosity multiplier.  The viscosity is computed
as  μ(𝜀̇′̅̅̅̅̅̅) = 𝑟𝑘 ⋅ 𝜀̇′̅̅̅̅̅̅(𝑟𝑛−1)  where  the  equivalent  deviatoric  strain  rate 
is 
̅̅̅̅̅̅ = √
𝜀′̇
[𝜀̇11
′ 2 + 𝜀̇22
′ 2 + 𝜀̇33
′ 2 + 2(𝜀̇12
′ 2 + 𝜀̇23
′ 2 + 𝜀̇31
′ 2)] 
Variable dynamic viscosity exponent . 
Characteristic length, 𝑙ci, of the internal turbulent domain. 
Internal  flow  mixing  length  polynomial  coefficients.    The  one-
parameter turbulent mixing length is computed as 
𝑙𝑐𝑖
⎡𝐶0 + 𝐶1 (1 −
⎢
⎣
) + ⋯ + 𝐶6 (1 −
𝑙m = 𝑙ci
𝑙𝑐𝑖
)
⎤ 
⎥
⎦
Characteristic length, 𝑙cx, of the external turbulent domain. 
External  flow  mixing  length  polynomial  coefficients.    If  𝑦 ≤ 𝑙cx
then the mixing length is computed as 𝑙𝑚 = [𝐷0 + 𝐷1𝑦 + 𝐷2𝑦2] 
External  flow  mixing  length  polynomial  coefficients.    If  𝑦 > 𝑙cx
then the mixing length is computed as 𝑙𝑚 = [𝐸0 + 𝐸1𝑦 + 𝐸2𝑦2] 
RO 
PC 
MULO 
MUHI 
RK 
RN 
LCI 
C0 - C6 
LCX 
D0 - D2 
E0 - E2 
Remarks: 
1.  The  null  material  must  be  used  with  an  equation  of-state.    Pressure  cutoff  is 
negative in tension.  A (deviatoric) viscous stress of the form 
′  
𝜎′𝑖𝑗 = 𝜇𝜀̇𝑖𝑗
𝑚2] ≈ [
is  computed  for  nonzero  𝜇  where  𝜀̇𝑖𝑗
namic viscosity with unit of [Pa × s]. 
[
] 
𝑚2 𝑠] [
′   is  the  deviatoric  strain  rate.   𝜇  is  the  dy-
2.  The  null  material  has  no  shear  stiffness  and  hourglass  control  must  be  used 
with care.  In some applications, the default hourglass coefficient might lead to 
significant  energy  losses.    In  general  for  fluid(s),  the  hourglass  coefficient  QM 
should be small (in the range 10−4 to 10−6 for the standard default IHQ choice). 
3.  The Null material has no yield strength and behaves in a fluid-like manner. 
4.  The pressure cut-off, PC, must be defined to allow for a material to “numerical-
ly”  cavitate.   In  other words,  when  a  material  undergoes  dilatation  above  cer-
tain  magnitude,  it  should  no  longer  be  able  to  resist  this  dilatation.    Since 
dilatation stress or pressure is negative, setting PC limit to a very small negative 
number would allow for the material to cavitate once the pressure in the mate-
rial goes below this negative value. 
5. 
If the viscosity exponent is less than 1.0, at very low equivalent strain rate, the 
viscosity can be artificially very high.  MULO is then used as the viscosity val-
ue.  
6.  Turbulence  is  treated  simply  by  considering  its  effects  on  viscosity.    Total 
effective  viscosity  is  the  sum  of  the  laminar  and  turbulent  viscosities, 
𝜇eff = 𝜇𝑙 + 𝜇𝑡 where 𝜇eff is the effective viscosity, and 𝜇𝑡 is the turbulent viscosi-
ty. 
7.  The  turbulent  viscosity  is  computed  based  on  the  Prandtl’s  Mixing  Length 
Model, 
𝜇𝑡 = ρ𝑙𝑚
2 |∇𝐯|
*MAT_ALE_INCOMPRESSIBLE 
See *MAT_160.
*MAT_ALE_HERSCHEL 
This may also be referred to as MAT_ALE_06.  This is the Herschel-Buckley model.  It is 
an  enhancement  to  the  power  law  viscosity  model  in  *MAT_ALE_VISCOUS(*MAT_-
ALE_03).  Two additional input parameters: the yield stress threshold and critical shear 
strain rate can be specified to model “rigid-like” material for low strain rates.   
It  allows  the  modeling  of  non-viscous  fluids  with  constant  or  variable  viscosity.    The 
variable  viscosity  is  a  function  of  an  equivalent  deviatoric  strain  rate.    All  *MAT_-
ALE_cards apply only to ALE element formulation. 
  Card 1 
1 
Variable 
MID 
Type 
I 
2 
RO 
F 
3 
PC 
F 
4 
5 
6 
7 
8 
MULO 
MUHI 
RK 
Not used 
RN 
F 
F 
F 
Defaults 
none 
none 
0.0 
0.0 
0.0 
0.0 
F 
0.0 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
GDOTC 
TAO0 
Type 
F 
F 
Default 
none 
none 
  VARIABLE   
DESCRIPTION
MID 
Material identification.  A unique number has to be chosen. 
RO 
PC 
Mass density. 
Pressure cutoff (≤ 0.0), .
VARIABLE   
DESCRIPTION
MULO 
There are 4 possible cases : 
1. 
2. 
3. 
4. 
If MULO = 0.0, then inviscid fluid is assumed. 
If  MULO > 0.0,  and  MUHI = 0.0  or  is  not  defined,  then 
this  is  the  traditional  constant  dynamic  viscosity  coeffi-
cient 𝜇. 
If MULO > 0.0, and MUHI > 0.0, then MULO and MUHI 
are  lower  and  upper  viscosity  limit  values  for  a  power-
law-like variable viscosity model. 
If  MULO  is  negative  (for  example,  MULO = -1),  then  a 
user-input  data  load  curve  (with  LCID = 1)  defining  dy-
namic  viscosity  as  a  function  of  equivalent  strain  rate  is
used. 
Upper  dynamic  viscosity  limit  (default = 0.0).    This  is  defined 
only if RK and RN are defined for the variable viscosity case. 
𝑘; consistency factor . 
𝑛; power law index . 
MUHI 
RK 
RN 
GDOTC 
𝛾̇𝑐; critical shear strain rate . 
TAO0 
𝜏0; yield stress . 
Remarks: 
1.  The  null  material  must  be  used  with  an  equation-of-state.    Pressure  cutoff  is 
negative in tension.  A (deviatoric) viscous stress of the form 
𝜎′𝑖𝑗 = 2𝜇𝜀′̇
𝑚2 𝑠] [
𝑚2] ~ [
is computed for nonzero 𝜇 where 𝜀′̇
𝑖𝑗 is the deviatoric strain rate.  𝜇 is the dy-
namic viscosity.  For example, in SI unit system, 𝜇 has a unit of [Pa*s]. 
𝑖𝑗 
] 
[
2.  The  null  material  has  no  shear  stiffness  and  hourglass  control  must  be  used 
with care.  In some applications, the default hourglass coefficient might lead to 
significant  energy  losses.    In  general  for  fluid(s),  the  hourglass  coefficient  QM 
should  be  small  (in  the  range  1.0E-4  to  1.0E-6  for  the  standard  default  IHQ 
choice).
3.  Null material has no yield strength and behaves in a fluid-like manner. 
4.  The pressure cut-off, PC, must be defined to allow for a material to “numerical-
ly”  cavitate.   In  other words,  when  a  material  undergoes  dilatation  above  cer-
tain  magnitude,  it  should  no  longer  be  able  to  resist  this  dilatation.    Since 
dilatation stress or pressure is negative, setting PC limit to a very small negative 
number would allow for the material to cavitate once the pressure in the mate-
rial goes below this negative value. 
5. 
If the viscosity exponent is less than 1.0, 𝑅𝑁 < 1.0, then 𝑅𝑁 − 1.0 < 0.0.  In this 
case,  at  very  low  equivalent  strain  rate,  the  viscosity  can  be  artificially  very 
high.  MULO is then used as the viscosity value. 
6.  The Herschel-Buckley model employs a large viscosity to model the “rigid-like” 
behavior for low shear strain rates (𝛾̇ < 𝛾̇𝑐).   
Power law is used once the yield stress is passed.   
𝜇 = 𝜇0 
μ(𝛾̇) =
𝜏0
𝛾̇
+ 𝑘(
𝛾̇
𝛾̇𝑐
)𝑛−1 
The shear strain rate is:  
𝛾̅̅̅̅̇ ≡ √
𝛾̇𝑖𝑗𝛾̇𝑖𝑗
= √2𝜀̇𝑖𝑗𝜀̇𝑖𝑗 = √4[𝜀̇12
2 + 𝜀̇23
2 + 𝜀̇31
2 ] + 2[𝜀̇11
2 + 𝜀̇22
2 ]
2 + 𝜀̇33
*MAT_SPH_VISCOUS 
This may also be referred to as MAT_SPH_01.  This “fluid-like” material model is very 
similar to Material Type 9 (*MAT_NULL).  It allows the modeling of viscous fluids with 
constant  or  variable  viscosity.    The  variable  viscosity  is  a  function  of  an  equivalent 
deviatoric strain rate.  If inviscid material is modeled, the deviatoric or viscous stresses 
are  zero,  and  the  equation  of  state  supplies  the  pressures  (or  diagonal  components  of 
the stress tensor).   
  Card 1 
1 
Variable 
MID 
Type 
I 
2 
RO 
F 
3 
PC 
F 
4 
5 
MULO 
MUHI 
F 
F 
6 
RK 
F 
7 
RC 
F 
8 
RN 
F 
Defaults 
none 
none 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
MID 
Material identification.  A unique number has to be chosen. 
RO 
PC 
Mass density. 
Pressure cutoff (≤ 0.0).  See Remark 4. 
MULO 
There are 4 possible cases : 
1. 
2. 
3. 
4. 
If MULO = 0.0, then inviscid fluid is assumed. 
If  MULO > 0.0,  and  MUHI = 0.0  or  is  not  defined,  then 
this  is  the  traditional  constant  dynamic  viscosity  coeffi-
cient 𝜇. 
If MULO > 0.0, and MUHI > 0.0, then MULO and MUHI 
are  lower  and  upper  viscosity  limit  values  for  a  power-
law-like variable viscosity model. 
If  MULO  is  negative  (for  example,  MULO = -1),  then  a 
user-input  data  load  curve  (with  LCID = 1)  defining  dy-
namic  viscosity  as  a  function  of  equivalent  strain  rate  is
used.
VARIABLE   
DESCRIPTION
MUHI 
There are 2 possible cases: 
5. 
6. 
If  MUHI < 0.0,  then  the  viscosity  can  be  defined  by  the 
user  in  the  file dyn21.F  with  a  routine  called  f3dm9sph_
userdefin.  The file is part of the general usermat package. 
If  MUHI > 0.0,  then  this  is  the  upper  dynamic  viscosity
limit  (default = 0.0).    This  is  defined  only  if  RK  and  RN 
are defined for the variable viscosity case. 
RK 
RC 
Variable dynamic viscosity multiplier.  See Remark 6. 
Option for Cross viscosity model:  See Remark 7. 
RC > 0.0:  Cross  viscosity  model  will  be  used  (overwrite  all
other options), values of MULO, MUHI, RK and RN
will  be  used  in  the  Cross  viscosity  model.    See  Re-
mark 7. 
RC ≤ 0.0:  other  viscosity  model  (decided  based  on  above
variables) will be used. 
RN 
Variable dynamic viscosity exponent.  See Remark 6. 
Remarks: 
1.  Deviatoric Viscous Stress.  The null material must be used with an equation-
of-state.  Pressure cutoff is negative in tension.  A (deviatoric) viscous stress of 
the form 
′  
′ = 2𝜇𝜀̇𝑖𝑗
𝜎𝑖𝑗
[
𝑚2] ~ [
𝑚2 𝑠] [
] 
is  computed  for  nonzero  𝜇  where  𝜀̇𝑖𝑗
namic viscosity.  For example, in SI unit system, 𝜇 has a unit of [Pa × s]. 
′   is  the  deviatoric  strain  rate.   𝜇  is  the  dy-
2.  Hourglass  Control  Issues.    The  null  material  has  no  shear  stiffness  and 
hourglass  control  must  be  used  with  care.    In  some  applications,  the  default 
hourglass  coefficient  might  lead  to  significant  energy  losses.    In  general  for 
fluid(s), the hourglass coefficient QM should be small (in the range 10−4 to 10−6 
for the standard default IHQ choice). 
3.  Null Material Properties.  Null material has no yield strength and behaves in a 
fluid-like manner.
4.  Numerical Cavitation.  The pressure cut-off, PC, must be defined to allow for a 
material to “numerically” cavitate.  In other words, when a material undergoes 
dilatation  above  certain  magnitude,  it  should  no  longer  be  able  to  resist  this 
dilatation.    Since  dilatation  stress  or  pressure  is  negative,  setting  PC  limit  to  a 
very  small  negative  number  would  allow  for  the  material  to  cavitate  once  the 
pressure in the material goes below this negative value. 
5. 
Issues with Small Values of Viscosity Exponent.  If the viscosity exponent is 
less than 1.0, RN < 1.0, then RN − 1.0 < 0.0.  In this case, at very low equivalent 
strain rate, the viscosity can be artificially very high.  MULO is then used as the 
viscosity value. 
6.  Empirical  Dynamic  Viscosity.    The  empirical  variable  dynamic  viscosity  is 
typically  modeled  as  a  function  of  equivalent  shear  rate  based  on  experimental 
data. 
For an incompressible fluid, this may be written equivalently as 
μ(𝛾̅̅̅̅̇ ′) = RK × 𝛾̅̅̅̅̇ ′(𝑅𝑁−1)
μ(𝜀̅
̇′) = RK × 𝜀̅
̇′(𝑅𝑁−1)
The “overbar” denotes a scalar equivalence.  The “dot” denotes a time deriva-
tive or rate effect.  And the “prime” symbol denotes deviatoric or volume pre-
serving components.  The equivalent shear rate components may be related to the 
basic definition of (small-strain) strain rate components as follows: 
𝜀̇𝑖𝑗 =
(
∂𝑢𝑖
∂𝑥𝑗
+
∂𝑢𝑗
∂𝑥𝑖
𝛾̇𝑖𝑗 = 2𝜀̇𝑖𝑗 
) ⇒ 𝜀̇𝑖𝑗
′ = 𝜀̇𝑖𝑗 − 𝛿𝑖𝑗 (
𝜀̇𝑘𝑘
) 
Typically, the 2nd invariant of the deviatoric strain rate tensor is defined as: 
The equivalent (small-strain) deviatoric strain rate is defined as:  
𝐼2𝜀̅
̇′ =
[𝜀̇𝑖𝑗
′ 𝜀̇𝑖𝑗
′ ] 
𝜀̅′̇ ≡ 2√𝐼2𝜀′̇ = √2[𝜀̇𝑖𝑗
′ 𝜀̇𝑖𝑗
′ ] = √4[𝜀̇12
′ 2 + 𝜀̇23
′ 2 + 𝜀̇31
′ 2] + 2[𝜀̇11
′ 2 + 𝜀̇22
′ 2 + 𝜀̇33
′ 2] 
In non-Newtonian literatures, the equivalent shear rate is sometimes defined as  
𝛾̅̅̅̅̇ ≡ √
𝛾̇𝑖𝑗𝛾̇𝑖𝑗
= √2𝜀̇𝑖𝑗𝜀̇𝑖𝑗 = √4[𝜀̇12
2 + 𝜀̇23
2 + 𝜀̇31
2 ] + 2[𝜀̇11
2 + 𝜀̇22
2 + 𝜀̇33
2 ] 
It  turns  out  that,  (a)  for  incompressible  materials  (𝜀̇𝑘𝑘 = 0),  and  (b)  the  shear 
′ , the equivalent shear rate is algebraical-
terms are equivalent when 𝑖 ≠ 𝑗→ 𝜀̇𝑖𝑗 = 𝜀̇𝑖𝑗
ly equivalent to the equivalent (small-strain) deviatoric strain rate. 
̇′ = 𝛾̅̅̅̅̇ ′ 
𝜀̅
7.  The  Cross  viscous  model  is  one  of  simplest  and  most  used  model  for  shear-
thinning  behavior,  i.e.,  the  fluid’s  viscosity  decreases  with  increasing  of  the 
local shear rate 𝛾̅̅̅̅̇, thus the dynamic viscosity μ is defined as a function of 𝛾̅̅̅̅̇: 
μ(𝛾̅̅̅̅̇ ′) = MUHI + (MULO − MUHI)/(1.0 + RK ∗ 𝛾̅̅̅̅̇ ′)𝑅𝑁−1 
Where RK and RN are two positive fitting parameters, and MULO, MUHI are 
the  limiting  values  of  the  viscosity  at  low  and  high  shear  rates,  respectively.  
RK, RN, MULO and MUHI are parameters from keyword input.
*MAT_S01 
This is Material Type 1 for discrete elements (*ELEMENT_DISCRETE).  This provides a 
translational or rotational elastic spring located between two nodes.  Only one degree of 
freedom is connected. 
3 
4 
5 
6 
7 
8 
  Card 1 
1 
Variable 
MID 
Type 
A8 
2 
K 
F 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
K 
Elastic stiffness (force/displacement) or (moment/rotation).
*MAT_DAMPER_VISCOUS 
This  is  Material  Type  2  for  discrete  elements  (*ELEMENT_DISCRETE).    This  material 
provides a linear translational or rotational damper located between two nodes.  Only 
one degree of freedom is then connected. 
3 
4 
5 
6 
7 
8 
  Card 1 
1 
Variable 
MID 
2 
DC 
Type 
A8 
F 
  VARIABLE   
DESCRIPTION
MID 
DC 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Damping 
constant 
ment/rotation rate). 
(force/displacement 
rate) 
or 
(mo-
*MAT_S03 
This  is  Material  Type  3  for  discrete  elements  (*ELEMENT_DISCRETE).    This  material 
provides  an  elastoplastic  translational  or  rotational  spring  with  isotropic  hardening 
located between two nodes.  Only one degree of freedom is connected. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
2 
K 
F 
3 
KT 
F 
4 
FY 
F 
5 
6 
7 
8 
  VARIABLE   
DESCRIPTION
MID 
K 
KT 
FY 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Elastic stiffness (force/displacement) or (moment/rotation). 
Tangent stiffness (force/displacement) or (moment/rotation). 
Yield (force) or (moment).
*MAT_SPRING_NONLINEAR_ELASTIC 
This  is  Material  Type  4  for  discrete  elements  (*ELEMENT_DISCRETE).    This  material 
provides  a  nonlinear  elastic  translational  and  rotational  spring  with  arbitrary  force 
versus displacement and moment versus rotation, respectively.  Optionally, strain rate 
effects  can  be  considered  through  a  velocity  dependent  scale  factor.    With  the  spring 
located between two nodes, only one degree of freedom is connected. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
LCD 
LCR 
Type 
A8 
I 
I 
  VARIABLE   
DESCRIPTION
MID 
LCD 
LCR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Load  curve  ID  describing  force  versus  displacement  or  moment
versus  rotation  relationship.    The  load  curve  must  define  the 
response in the negative and positive quadrants and pass through
point (0,0). 
Optional load curve describing scale factor on force or moment as 
a function of relative velocity or.  rotational velocity, respectively.
*MAT_DAMPER_NONLINEAR_VISCOUS 
This  is  Material  Type  5  for  discrete  elements  (*ELEMENT_DISCRETE).    This  material 
provides  a  viscous  translational  damper  with  an  arbitrary  force  versus  velocity 
dependency,  or  a  rotational  damper  with  an  arbitrary  moment  versus  rotational 
velocity dependency.  With the damper located between two nodes, only one degree of 
freedom is connected. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
LCDR 
Type 
A8 
I 
  VARIABLE   
DESCRIPTION
MID 
LCDR 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
identification  describing 
force  versus  rate-of-
Load  curve 
displacement  relationship  or  a  moment  versus  rate-of-rotation 
relationship.    The  load  curve  must  define  the  response  in  the 
negative and positive quadrants and pass through point (0,0).
*MAT_SPRING_GENERAL_NONLINEAR 
This  is  Material  Type  6  for  discrete  elements  (*ELEMENT_DISCRETE).    This  material 
provides  a  general  nonlinear  translational  or  rotational  spring  with  arbitrary  loading 
and unloading definitions.  Optionally, hardening or softening can be defined.  With the 
spring located between two nodes, only one degree of freedom is connected. 
  Card 1 
1 
2 
3 
4 
Variable 
MID 
LCDL 
LCDU 
BETA 
5 
TYI 
6 
CYI 
7 
8 
Type 
A8 
I 
I 
F 
F 
F 
  VARIABLE   
DESCRIPTION
MID 
LCDL 
LCDU 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Load  curve 
force/torque  versus
displacement/rotation relationship for loading, see Figure M26-1.
identification  describing 
identification  describing 
Load  curve 
force/torque  versus
displacement/rotation  relationship  for  unloading,  see  Figure 
M119-1. 
BETA 
Hardening parameter, 𝛽: 
EQ.0.0:  Tensile  and  compressive  yield  with  strain  softening
(negative or zero slope allowed in the force versus dis-
placement.    load  curves).   TYI  and  CYI  are not  imple-
mented for this option. 
NE.0.0:  Kinematic hardening without strain softening. 
EQ.1.0:  Isotropic hardening without strain softening. 
Initial yield force in tension ( > 0) 
Initial yield force in compression ( < 0) 
TYI 
CYI 
Remarks: 
Load  curve  points  are  in  the  format  (displacement,  force  or  rotation,  moment).    The 
points must be in order starting with the most negative (compressive) displacement or
rotation  and  ending  with  the  most  positive  (tensile)  value.    The  curves  need  not  be 
symmetrical. 
The displacement origin of the “unloading” curve is arbitrary, since it will be shifted as 
necessary  as  the  element  extends  and  contracts.    On  reverse  yielding  the  “loading” 
curve will also be shifted along the displacement re or.  rotation axis.  The initial tensile 
and compressive  
Yield forces (TYI and CYI) define a range within which the element remains elastic (i.e.  
the “loading” curve is used for both loading and unloading).  If at any time the force in 
the  element  exceeds  this  range,  the  element  is  deemed  to  have  yielded,  and  at  all 
subsequent times the “unloading” curve is used for unloading 
Figure MS6-1.  General Nonlinear material for discrete elements
*MAT_SPRING_MAXWELL 
This  is  Material  Type  7  for  discrete  elements  (*ELEMENT_DISCRETE).    This  material 
provides  a  three  Parameter  Maxwell  Viscoelastic  translational  or  rotational  spring.  
Optionally, a cutoff time with a remaining constant force/moment can be defined. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
2 
K0 
F 
3 
KI 
F 
4 
BETA 
F 
Default 
5 
TC 
F 
1020 
6 
FC 
F 
0 
7 
8 
COPT 
F 
0 
  VARIABLE   
DESCRIPTION
MID 
K0 
KI 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
𝐾0, short time stiffness 
𝐾∞, long time stiffness 
BETA 
Decay parameter. 
TC 
FC 
Cut  off  time.    After  this  time  a  constant  force/moment  is
transmitted. 
Force/moment after cutoff time 
COPT 
Time implementation option: 
EQ.0: incremental time change, 
NE.0:  continuous time change. 
Remarks: 
The time varying stiffness K(t) may be described in terms of the input parameters as 
𝐾(𝑇) = 𝐾∞ + (𝐾0 − 𝐾∞)exp (−𝛽t) 
This  equation  was  implemented  by  Schwer  [1991]  as  either  a  continuous  function  of 
time  or  incrementally  following  the  approach  of  Herrmann  and  Peterson  [1968].    The 
continuous  function  of  time  implementation  has  the  disadvantage  of  the  energy
absorber’s  resistance  decaying  with  increasing  time  even  without  deformation.    The 
advantage of the incremental implementation is that an energy absorber must undergo 
some deformation before its resistance decays, i.e., there is no decay until impact, even 
in  delayed  impacts.    The  disadvantage  of  the  incremental  implementation  is  that  very 
rapid decreases in resistance cannot be easily matched.
*MAT_SPRING_INELASTIC 
This  is  Material  Type  8  for  discrete  elements  (*ELEMENT_DISCRETE).    This  material 
provides  an  inelastic  tension  or  compression  only,  translational  or  rotational  spring.  
Optionally,  a  user-specified  unloading  stiffness  can  be  taken  instead  of  the  maximum 
loading stiffness. 
  Card 1 
1 
2 
Variable 
MID 
LCFD 
Type 
A8 
I 
3 
KU 
F 
4 
CTF 
F 
5 
6 
7 
8 
  VARIABLE   
DESCRIPTION
MID 
LCFD 
KU 
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Load  curve 
identification  describing  arbitrary  force/torque
versus  displacement/rotation  relationship.    This  curve  must  be
defined in the positive force-displacement quadrant regardless of 
whether the spring acts in tension or compression. 
Unloading  stiffness  (optional).    The  maximum  of  KU  and  the
maximum  loading  stiffness  in  the  force/displacement  or  the
moment/rotation curve is used for unloading. 
CTF 
Flag for compression/tension: 
EQ.-1.0:  tension only, 
EQ.0.0:  default is set to 1.0, 
EQ.1.0:  compression only.
*MAT_SPRING_TRILINEAR_DEGRADING 
This is Material Type 13 for discrete elements (*ELEMENT_DISCRETE).  This material 
allows  concrete  shearwalls  to  be  modeled  as  discrete  elements  under  applied  seismic 
loading.    It  represents  cracking  of  the  concrete,  yield  of  the  reinforcement  and  overall 
failure.  Under cyclic loading, the stiffness of the spring degrades but the strength does 
not. 
  Card 1 
1 
2 
Variable 
MID 
DEFL1 
Type 
A8 
F 
3 
F1 
F 
4 
DEFL2 
F 
5 
F2 
F 
6 
DEFL3 
F 
7 
F3 
F 
8 
FFLAG 
F 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
DEFL1 
Deflection at point where concrete cracking occurs. 
F1 
Force corresponding to DEFL1 
DEFL2 
Deflection at point where reinforcement yields 
F2 
Force corresponding to DEFL2 
DEFL3 
Deflection at complete failure 
F3 
Force corresponding to DEFL3 
FFLAG 
Failure flag.
*MAT_SPRING_SQUAT_SHEARWALL 
This is Material Type 14 for discrete elements (*ELEMENT_DISCRETE).  This material 
allows  squat  shear  walls  to  be  modeled  using  discrete  elements.    The  behavior  model 
captures  concrete  cracking,  reinforcement  yield,  ultimate  strength  followed  by 
degradation of strength finally leading to collapse. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
A14 
B14 
C14 
D14 
E14 
LCID 
FSD 
Type 
A8 
F 
F 
F 
F 
F 
I 
F 
  VARIABLE   
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
Material coefficient 𝐴 
Material coefficient 𝐵 
Material coefficient 𝐶 
Material coefficient 𝐷 
Material coefficient 𝐸 
Load curve ID referencing the maximum strength envelope curve
Sustained strength reduction factor 
MID 
A14 
B14 
C14 
D14 
E14 
LCID 
FSD 
Remarks: 
Material coefficients 𝐴, 𝐵, 𝐶 and 𝐷 are empirically defined constants used to define the 
shape  of  the  polynomial  curves  which  govern  the  cyclic  behavior  of  the  discrete 
element.    A  different  polynomial  relationship  is  used  to  define  the  loading  and 
unloading  paths  allowing  energy  absorption  through  hysteresis.   Coefficient  E  is  used 
in the definition of the path used to “jump” from the loading path to the unloading path 
(or vice versa) where a full hysteresis loop is not completed.  The load curve referenced 
is  used  to  define  the  force  displacement  characteristics  of  the  shear  wall  under 
monotonic loading.  This curve is the basis to which the polynomials defining the cyclic 
behavior  refer  to.    Finally,  on  the  second  and  subsequent  loading  /  unloading  cycles,
the shear wall will have reduced strength.   The variable FSD is the sustained strength 
reduction factor.
*MAT_SPRING_MUSCLE 
This is Material Type 15 for discrete elements (*ELEMENT_DISCRETE).  This material 
is  a  Hill-type  muscle  model  with  activation.    It  is  for  use  with  discrete  elements.    The 
LS-DYNA implementation is due to Dr.  J.  A.  Weiss. 
  Card 1 
1 
Variable 
MID 
Type 
A8 
2 
L0 
F 
3 
VMAX 
F 
Default 
1.0 
4 
SV 
F 
1.0 
5 
A 
F 
6 
FMAX 
F 
7 
TL 
F 
8 
TV 
F 
1.0 
1.0 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FPE 
LMAX 
KSH 
Type 
F 
F 
F 
Default 
0.0 
  VARIABLE   
MID 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
characters must be specified. 
L0 
Initial muscle length, 𝐿0. 
VMAX 
Maximum CE shortening velocity, 𝑉max. 
SV 
Scale factor, 𝑆𝑣, for 𝑉max vs.  active state. 
LT.0:  absolute value gives load curve ID 
GE.0:  constant value of 1.0 is used 
A 
Activation level vs.  time function 𝑎(𝑡). 
LT.0:  absolute value gives load curve ID 
GE.0:  constant value of A is used
VARIABLE   
DESCRIPTION
FMAX 
Peak isometric force, 𝐹max. 
TL 
Active tension vs.  length function, 𝑓TL(𝐿). 
LT.0:  absolute value gives load curve ID 
GE.0:  constant value of 1.0 is used 
TV 
Active tension vs.  velocity function, 𝑓TV(𝑉). 
LT.0:  absolute value gives load curve ID 
GE.0:  constant value of 1.0 is used 
FPE 
Force vs.  length function, 𝑓PE, for parallel elastic element. 
LT.0:  absolute value gives load curve ID 
EQ.0:  exponential function is used  
GT.0:  constant value of 0.0 is used 
Relative length when 𝐹PE reaches 𝐹max.  Required if 𝐹PE above. 
Constant,  𝐾sh,  governing  the  exponential  rise  of𝐹PE.    Required  if 
𝐹PE above. 
LMAX 
KSH 
Remarks: 
The  material  behavior  of  the  muscle  model  is  adapted  from  the  original  model 
proposed by Hill [1938].  Reviews of this model and extensions can be found in Winters 
[1990] and Zajac [1989].  The most basic Hill-type muscle model consists of a contractile 
element (CE) and a parallel elastic element (PE) (Figure MS15-1).  An additional series 
elastic element (SEE) can be added to represent tendon compliance. 
The  main  assumptions  of  the  Hill  model  are  that  the  contractile  element  is  entirely 
stress  free  and  freely  distensible  in  the  resting  state,  and  is  described  exactly  by  Hill’s 
equation  (or  some  variation).    When  the  muscle  is  activated,  the  series  and  parallel 
elements  are  elastic,  and  the  whole  muscle  is  a  simple  combination  of  identical 
sarcomeres in series and parallel.  The main criticism of Hill’s model is that the division 
of forces between the parallel elements and the division of extensions between the series 
elements  is  arbitrary,  and  cannot  be  made  without  introducing  auxiliary  hypotheses.  
However,  these  criticisms  apply  to  any  discrete  element  model.    Despite  these 
limitations, the Hill model has become extremely useful for modeling musculoskeletal 
dynamics, as illustrated by its widespread use today.
a(t)
SEE
FM
FCE
FPE
LM
vM
CE
FM
LM
PE
Figure  MS15-1.  Discrete model for muscle contraction dynamics, based on a
Hill-type  representation.    The  total  force  is  the  sum  of  passive  force  𝐹PE  and 
active  force  𝐹CE.    The  passive  element  (PE)  represents  energy  storage  from
muscle  elasticity,  while  the  contractile  element  (CE)  represents  force 
generation  by  the  muscle.    The  series  elastic  element  (SEE),  shown  in  dashed
lines,  is  often  neglected  when  a  series  tendon  compliance  is  included.    Here,
𝑎(𝑡)  is  the  activation  level,  𝐿M  is  the  length  of  the  muscle,  and  𝑉M  is  the 
shortening velocity of the muscle. 
When the contractile element (CE) of the Hill model is inactive, the entire resistance to 
elongation is provided by the PE element and the tendon load-elongation behavior.  As 
activation is increased, force then passes through the CE side of the parallel Hill model, 
providing  the  contractile  dynamics.    The  original  Hill  model  accommodated  only  full 
activation - this limitation is circumvented in the present implementation by using the 
modification  suggested  by  Winters  (1990).   The  main  features  of his  approach  were  to 
realize that the CE force-velocity input force equals the CE tension-length output force.  
This yields a three-dimensional curve to describe the force-velocity-length relationship 
of  the  CE.    If  the  force-velocity  y-intercept  scales  with  activation,  then  given  the 
activation, length and velocity, the CE force can be determined. 
Without the SEE, the total force in the muscle FM is the sum of the force in the CE and 
the PE because they are in parallel: 
𝐹M = 𝐹PE + 𝐹CE 
The relationships defining the force generated by the CE and PE as a function of 𝐿M, 𝑉M 
and 𝑎(𝑡) are often scaled by 𝐹max, the peak isometric force (p.  80, Winters 1990), 𝐿0, the 
initial length of the muscle (p.  81, Winters 1990), and 𝑉max, the maximum unloaded CE 
shortening  velocity  (p.    80,  Winters  1990).    From  these,  dimensionless  length  and 
velocity can be defined: 
𝐿 =
𝐿M
𝐿0
, 
𝑉 =
𝑉M
𝑉max × 𝑆𝑣[𝑎(𝑡)]
Here, 𝑆𝑣 scales the maximum CE shortening velocity 𝑉max and changes with activation 
level 𝑎(𝑡).  This has been suggested by several researchers, i.e.  Winters and Stark [1985].  
The activation level specifies the level of muscle stimulation as a function of time.  Both 
have  values  between  0  and  1.    The  functions  𝑆𝑣(𝑎(𝑡))  and  𝑎(𝑡)  are  specified  via  load 
curves  in  LS-DYNA,  or  default  values  of  𝑆v = 1  and  𝑎(𝑡) = 0  are  used.    Note  that  𝐿  is 
always positive and that 𝑉 is positive for lengthening and negative for shortening. 
The relationship between 𝐹CE, 𝑉 and 𝐿 was proposed by Bahler et al.  [1967].  A three-
dimensional  relationship  between  these  quantities  is  now  considered  standard  for 
computer implementations of Hill-type muscle models [Winters 1990].  It can be written 
in dimensionless form as: 
𝐹CE = 𝑎(𝑡) × 𝐹max × 𝑓TL(𝐿) × 𝑓TV(𝑉) 
Here, 𝑓TL(𝐿) and 𝑓TV(𝑉) are the tension-length and tension-velocity functions for active 
skeletal muscle.  Thus, if current values of 𝐿M, 𝑉M, and 𝑎(𝑡) are known, then 𝐹CE can be 
determined (Figure MS15-1). 
The  force  in  the  parallel  elastic  element  𝐹PE  is  determined  directly  from  the  current 
length of the muscle using an exponential relationship [Winters 1990]: 
𝑓PE =
𝐹PE
𝐹MAX
=
⎧
{
{
⎨
{
{
⎩
𝐿 ≤ 1
exp(𝐾sh) − 1
{exp [
𝐾sh
𝐿max
(𝐿 − 1)] − 1} 𝐿 > 1
Here,  𝐿max  is  the  relative  length  at  which  the  force  𝐹max  occurs,  and  𝐾sh  is  a 
dimensionless  shape  parameter  controlling  the  rate  of  rise  of  the  exponential.  
Alternatively,  the  user  can  define  a  custom  𝑓PE  curve  giving  tabular  values  of 
normalized force versus dimensionless length as a load curve. 
For  computation  of  the  total  force  developed  in  the  muscle  𝐹M,  the  functions  for  the 
tension-length 𝑓TL(𝐿) and force-velocity fTV relationships used in the Hill element must 
be  defined.    These  relationships  have  been  available  for  over  50  years,  but  have  been 
refined  to  allow  for  behavior  such  as  active  lengthening.    The  active  tension-length 
curve 𝑓TL(𝐿) describes the fact that isometric muscle force development is a function of 
length, with the maximum force occurring at an optimal length.  According to Winters, 
this  optimal  length  is  typically  around 𝐿 = 1.05,  and  the  force  drops  off  for  shorter  or 
longer  lengths,  approaching  zero  force  for  𝐿 = 0.4  and  𝐿 = 1.5.    Thus  the  curve  has  a 
bell-shape.    Because  of  the  variability  in  this  curve  between  muscles,  the  user  must 
specify the function 𝑓𝑇𝐿(𝐿) via a load curve, specifying pairs of points representing the 
normalized  force  (with  values  between  0  and  1)  and  normalized  length  𝐿.    See  Figure 
MS15-2.
Figure MS15-2.  Typical normalized tension-length (TL) and tension-velocity 
(TV) curves for skeletal muscle. 
The active tension-velocity relationship 𝑓TV(𝑉) used in the muscle model is mainly due 
to  the  original  work  of  Hill.    Note  that  the  dimensionless  velocity  𝑉 is  used.    When 
𝑉 = 0,  the  normalized  tension  is  typically  chosen  to  have  a  value  of  1.0.    When  𝑉  is 
greater  than  or  equal  to  0,  muscle  lengthening  occurs.    As  𝑉  increases,  the  function  is 
typically  designed  so  that  the  force  increases  from  a  value  of  1.0  and  asymptotes 
towards a value near 1.4 ass shown in Figure MS15-2.  When 𝑉 is less than zero, muscle 
shortening  occurs  and  the  classic  Hill  equation  hyperbola  is  used  to  drop  the 
normalized tension to 0 as shown in Figure MS15-2.  The user must specify the function 
𝑓TV(𝑉) via a load curve, specifying pairs of points representing the normalized tension 
(with values between 0 and 1) and normalized velocity 𝑉
Available options include: 
2D 
Purpose:  Define a seat belt material. 
*MAT_B01 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
Variable 
MID 
MPUL 
LLCID 
ULCID 
LMIN 
CSE 
DAMP 
Type 
A8 
Default 
0 
F 
0. 
I 
0 
I 
0 
F 
F 
F 
0.0 
0.0 
0.0 
0.0 
8 
E 
F 
Bending/Compression Parameter Card.  Additional card for E.GT.0. 
  Card 2 
Variable 
Type 
1 
A 
F 
2 
I 
F 
3 
J 
F 
Default 
0.0 
0.0 
2*I 
4 
AS 
F 
A 
8 
5 
F 
F 
6 
M 
F 
7 
R 
F 
1.0e20  1.0e20 
0.05 
Additional card for 2D option 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
P1DOFF 
Type 
Default 
I
VARIABLE   
DESCRIPTION
MID 
MPUL 
LLCID 
ULCID 
LMIN 
CSE 
Belt material number.  A unique number or label not exceeding 8
characters must be specified. 
Mass per unit length 
Curve or table ID for loading.  LLCID can be either a single curve
(force  vs.    engineering  strain),  or  a  table  defining  a  set  of  strain-
rate dependent loading curves. 
Load  curve  identification  for  unloading  (force  vs.    engineering
strain). 
Minimum  length  (for  elements  connected  to  slip  rings  and
retractors), see notes below. 
Optional  compressive  stress  elimination  option  which  applies  to 
shell elements only (default 0.0): 
EQ.0.0: eliminate compressive stresses in shell fabric 
EQ.1.0: do  not  eliminate  compressive  stresses.    This  option
should not be used if retractors and slip rings are pre-
sent in the model. 
EQ.2.0: whether  or  not  compressive  stress  is  eliminated  is
decided by LS-DYNA automatically, recommended for 
shell belt.  
DAMP 
Optional  Rayleigh  damping  coefficient,  which  applies  to  shell
elements  only.    A  coefficient  value  of  0.10  is  the  default
corresponding to 10% of critical damping.  Sometimes smaller or
larger values work better. 
E 
A 
I 
J 
Young’s  modulus  for  bending/compression  stiffness,  when
positive the optional card is invoked.  See remarks. 
Cross  sectional  area  for  bending/compression  stiffness,  see
remarks. 
Area  moment  of  inertia  for  bending/compression  stiffness,  see
remarks. 
Torsional  constant 
remarks. 
for  bending/compression  stiffness,  see
AS 
Shear area for bending/compression stiffness, see remarks.
VARIABLE   
DESCRIPTION
Maximum force in compression/tension, see remarks. 
Maximum torque, see remarks. 
Rotational mass scaling factor, see remarks. 
Part ID offset for internally created 1D, bar-type, belt parts for 2D 
seatbelt  of  this  material,  i.e.,  the  IDs  of  newly  created  1D  belt
parts will be P1DOFF + 1, P1DOFF + 2, …  If zero, the maximum 
ID of user-defined parts is used as the part ID offset. 
F 
M 
R 
P1DOFF 
Remarks: 
Each  belt  material  defines  stretch  characteristics  and  mass  properties  for  a  set  of  belt 
elements.    The  user  enters  a  load  curve  for  loading,  the  points  of  which  are  (Strain, 
Force).  Strain is defined as engineering strain, i.e. 
Strain =
current length
initial length
− 1.0 
Another similar curve is entered to describe the unloading behavior.  Both load curves 
should  start  at  the  origin  (0,0)  and  contain  positive  force  and  strain  values  only.    The 
belt  material  is  tension  only  with  zero  forces  being  generated  whenever  the  strain 
becomes negative.  The first non-zero point on the loading curve defines the initial yield 
point of the material.  On unloading, the unloading curve is shifted along the strain axis 
until it crosses the loading curve at the “yield” point from which unloading commences.  
If the initial yield has  not yet been exceeded or if the origin of the (shifted) unloading 
curve is at negative strain, the original loading curves will be used for both loading and 
unloading.  If the strain is less than the strain at the origin of the unloading curve, the 
belt is slack and no force is generated.  Otherwise, forces will then be determined by the 
unloading curve for unloading and reloading until the strain again exceeds yield after 
which the loading curves will again be used. 
A  small  amount  of  damping  is  automatically  included.    This  reduces  high  frequency 
oscillation,  but,  with  realistic  force-strain  input  characteristics  and  loading  rates,  does 
not  significantly  alter  the  overall  forces-strain  performance.    The  damping  forced 
opposes the relative motion of the nodes and is limited by stability: 
𝐷 =
0.1 ×  mass × relative velocity
 time step size
In  addition,  the  magnitude  of  the  damping  force  is  limited  to  one-tenth  of  the  force 
calculated  from  the  force-strain  relationship  and  is  zero  when  the  belt  is  slack.  
Damping forces are not applied to elements attached to sliprings and retractors.
The  user  inputs  a  mass  per  unit  length  that  is  used  to  calculate  nodal  masses  on 
initialization. 
A  “minimum  length”  is  also  input.    This  controls  the  shortest  length  allowed  in  any 
element and determines when an element passes through sliprings or are absorbed into 
the retractors.  One tenth of a typical initial element length is usually a good choice. 
Bending and Compression Stiffness for 1D Elements: 
Since  these  elements  do  not  possess  any  bending  or  compression  stiffness,  when  belts 
are  used  in  an  implicit  analysis,  dynamic  analysis  is  mandatory.    However,  one 
dimensional  belt  elements  can  be  used  in  implicit  statics  by  associating  them  with 
bending/compression  properties  as  per  the  first  optional  card.    Two  dimensional  belt 
elements are not supported with this feature. 
To achieve bending and compression stiffness in 1D belts the belt element is overlayed 
with  a  Belytschko-Schwer  beam  element   with circular cross section.  
These elements have 6 degrees of freedom including rotational degrees of freedom.  The 
material used in this context is an elastic-ideal-plastic material where the elastic part is 
governed  by  the  Young’s  modulus  E.    Two  yield  values,  F  being  the  maximum 
compression/tension  force  and  M  being  the  maximum  torque,  are  used  as  upper 
bounds  for  the  resultants.    The  bending/compression  forces  and  moments  from  this 
contribution  are  accumulated  to  the  force  from  the  seatbelt  itself.    Since  the  main 
purpose is to eliminate the singularities in bending and compression, it is recommend-
ed to choose the bending and compression properties in the optional card carefully so 
as to not significantly influence the overall response. 
For  the  sake  of  completeness,  this  feature  is  also  supported  by  the  explicit  integrator; 
therefore, a rotational nodal mass is needed.  Each of the two nodes of an element gets a 
contribution  from  the  belt  that  is  calculated  as  RMASS = R × (MASS/2) × I/A,  where 
MASS indicates the total translational mass of the belt element and R is a scaling factor 
input  by  the  user.    The  translational  mass  is  not  modified.    The  bending  and 
compression properties do not affect the stable time step.  If the belts are used without 
sliprings,  then  incorporating  this  feature  is  virtually  equivalent  to  adding  Belytschko-
Schwer beams on top of conventional belt elements as part of a modelling strategy.  If 
sliprings  are  used,  this  feature  is  necessary  to  properly  support  the  flow  of  material 
through the sliprings and swapping of belt elements across sliprings.  Retractors cannot 
be used with this feature.
*MAT_THERMAL_{OPTION} 
Available options include: 
ISOTROPIC 
ORTHOTROPIC 
ISOTROPIC_TD 
ORTHOTROPIC_TD 
DISCRETE_BEAM 
CWM 
ORTHOTROPIC_TD_LC 
ISOTROPIC_PHASE_CHANGE 
ISOTROPIC_TD_LC 
USER_DEFINED 
The  *MAT_THERMAL_cards  allow  thermal  properties  to  be  defined  in  coupled 
structural/thermal  and  thermal  only  analyses,  see  *CONTROL_SOLUTION.    Thermal 
properties must be defined for all elements in such analyses.  
Thermal material properties are specified by a thermal material ID number (TMID), this 
number is independent of the material ID number (MID) defined on all other *MAT_… 
property cards.  In the same analysis identical TMID and MID numbers may exist.  The 
TMID and MID numbers are related through the *PART card.
*MAT_THERMAL_ISOTROPIC 
This is thermal material type 1.  It allows isotropic thermal properties to be defined. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TMID 
TRO 
TGRLC 
TGMULT 
TLAT 
HLAT 
F 
3 
F 
4 
F 
5 
F 
6 
7 
8 
Type 
A8 
F 
  Card 2 
Variable 
1 
HC 
Type 
F 
2 
TC 
F 
  VARIABLE   
TMID 
DESCRIPTION
Thermal  material  identification.    A  unique  number  or  label  not
exceeding 8 characters must be specified. 
TRO 
Thermal density: 
EQ.0.0:  default to structural density. 
TGRLC 
Thermal generation rate curve number, see *DEFINE_CURVE: 
GT.0:  function versus time, 
EQ.0:  use constant multiplier value, TGMULT, 
LT.0:  function versus temperature. 
TGMULT 
Thermal generation rate multiplier: 
EQ.0.0:  no heat generation. 
Phase change temperature 
Latent heat 
Specific heat 
Thermal conductivity 
TLAT 
HLAT 
HC 
TC
*MAT_THERMAL_ORTHOTROPIC 
This is thermal material type 2.  It allows orthotropic thermal properties to be defined. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TMID 
TRO 
TGRLC 
TGMULT 
AOPT 
TLAT 
HLAT 
Type 
A8 
F 
F 
F 
F 
5 
5 
A2 
F 
5 
F 
6 
6 
A3 
F 
6 
F 
7 
8 
7 
8 
7 
8 
4 
K3 
F 
4 
A1 
F 
4 
2 
K1 
F 
2 
YP 
F 
2 
D2 
F 
3 
K2 
F 
3 
ZP 
F 
3 
D3 
F 
  Card 2 
Variable 
1 
HC 
Type 
F 
  Card 3 
Variable 
1 
XP 
Type 
F 
  Card 4 
Variable 
1 
D1 
Type 
F 
  VARIABLE   
TMID 
DESCRIPTION
Thermal  material  identification.    A  unique  number  or  label  not
exceeding 8 characters must be specified. 
TRO 
Thermal density: 
EQ.0.0:  default to structural density.
*MAT_THERMAL_ORTHOTROPIC 
DESCRIPTION
TGRLC 
Thermal generation rate curve number, see *DEFINE_CURVE: 
GT.0:  function versus time, 
EQ.0:  use constant multiplier value, TGMULT, 
LT.0:  function versus temperature. 
TGMULT 
Thermal generation rate multiplier: 
EQ.0.0:  no heat generation. 
AOPT 
Material axes definition: 
EQ.0.0:  locally  orthotropic  with  material  axes  by  element
nodes N1, N2 and N4, 
EQ.1.0:  locally orthotropic with material axes determined by a
point in space and global location of element center, 
EQ.2.0:  globally orthotropic with material axes determined by
TLAT 
HLAT 
HC 
K1 
K2 
K3 
vectors. 
Phase change temperature 
Latent heat 
Specific heat 
Thermal conductivity K1 in local x-direction 
Thermal conductivity K2 in local y-direction 
Thermal conductivity K3 in local z-direction 
XP, YP, ZP 
Define coordinate of point p for AOPT = 1 
A1, A2, A3 
Define components of vector a for AOPT = 2 
D1, D2, D3 
Define components of vector v for AOPT = 2
*MAT_THERMAL_ISOTROPIC_TD 
This is thermal material type 3.  It allows temperature dependent isotropic properties to 
be  defined.    The  temperature  dependency  is  defined  by  specifying  a  minimum  of  two 
and  a  maximum  of  eight  data  points.    The  properties  must  be  defined  for  the 
temperature range that the material will see in the analysis. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TMID 
TRO 
TGRLC 
TGMULT 
TLAT 
HLAT 
Type 
A8 
F 
F 
F 
F 
F 
  Card 2 
Variable 
1 
T1 
Type 
F 
  Card 3 
Variable 
1 
C1 
Type 
F 
  Card 4 
Variable 
1 
K1 
Type 
F 
  VARIABLE   
TMID 
2 
T2 
F 
2 
C2 
F 
2 
K2 
F 
3 
T3 
F 
3 
C3 
F 
3 
K3 
F 
4 
T4 
F 
4 
C4 
F 
4 
K4 
F 
5 
T5 
F 
5 
C5 
F 
5 
K5 
F 
6 
T6 
F 
6 
C6 
F 
6 
K6 
F 
7 
T7 
F 
7 
C7 
F 
7 
K7 
F 
8 
T8 
F 
8 
C8 
F 
8 
K8 
F 
DESCRIPTION
Thermal  material  identification.    A  unique  number  or  label  not
exceeding 8 characters must be specified.
*MAT_THERMAL_ISOTROPIC_TD 
DESCRIPTION
TRO 
Thermal density: 
EQ.0.0 default to structural density. 
TGRLC 
Thermal generation rate curve number, see *DEFINE_CURVE: 
GT.0:  function versus time, 
EQ.0:  use constant multiplier value, TGMULT, 
LT.0:  function versus temperature. 
TGMULT 
Thermal generation rate multiplier: 
EQ.0.0:  no heat generation. 
TLAT 
HLAT 
Phase change temperature 
Latent heat 
T1, …, T8 
Temperatures: T1, ..., T8 
C1, …, C8 
Specific heat at: T1, …, T8 
K1, …, K8 
Thermal conductivity at: T1, …, T8
*MAT_THERMAL_ORTHOTROPIC_TD 
This is thermal material type 4.  It allows temperature dependent orthotropic properties 
to be defined.  The temperature dependency is defined by specifying a minimum of two 
and  a  maximum  of  eight  data  points.    The  properties  must  be  defined  for  the 
temperature range that the material will see in the analysis. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TMID 
TRO 
TGRLC 
TGMULT 
AOPT 
TLAT 
HLAT 
Type 
A8 
F 
F 
F 
F 
F 
F 
  Card 2 
Variable 
1 
T1 
Type 
F 
  Card 3 
Variable 
1 
C1 
Type 
F 
  Card 4 
1 
2 
T2 
F 
2 
C2 
F 
2 
3 
T3 
F 
3 
C3 
F 
3 
4 
T4 
F 
4 
C4 
F 
4 
5 
T5 
F 
5 
C5 
F 
5 
6 
T6 
F 
6 
C6 
F 
6 
7 
T7 
F 
7 
C7 
F 
7 
8 
T8 
F 
8 
C8 
F 
8 
Variable 
(K1)1 
(K1)2 
(K1)3 
(K1)4 
(K1)5 
(K1)6 
(K1)7 
(K1)8 
Type 
F 
  Card 5 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
F 
7 
F 
8 
Variable 
(K2)1 
(K2)2 
(K2)3 
(K2)4 
(K2)5 
(K2)6 
(K2)7 
(K2)8 
Type 
F 
F 
F 
F 
F 
F 
F
Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
(K3)1 
(K3)2 
(K3)3 
(K3)4 
(K3)5 
(K3)6 
(K3)7 
(K3)8 
Type 
F 
F 
F 
F 
F 
F 
F 
7 
F 
8 
7 
8 
4 
A1 
F 
4 
5 
A2 
F 
5 
6 
A3 
F 
6 
2 
YP 
F 
2 
D2 
F 
3 
ZP 
F 
3 
D3 
F 
  Card 7 
Variable 
1 
XP 
Type 
F 
  Card 8 
Variable 
1 
D1 
Type 
F 
  VARIABLE   
TMID 
DESCRIPTION
Thermal  material  identification.    A  unique  number  or  label  not
exceeding 8 characters must be specified. 
TRO 
Thermal density: 
EQ.0.0:  default to structural density. 
TGRLC 
Thermal generation rate curve number, see *DEFINE_CURVE: 
GT.0:  function versus time, 
EQ.0:  use constant multiplier value, TGMULT, 
LT.0:  function versus temperature. 
TGMULT 
Thermal generation rate multiplier: 
EQ.0.0:  no heat generation.
VARIABLE   
AOPT 
DESCRIPTION
Material  axes  definition:  : 
EQ.0.0:  locally  orthotropic  with  material  axes  by  element
nodes N1, N2 and N4, 
EQ.1.0:  locally orthotropic with material axes determined by a
point in space and global location of element center, 
EQ.2.0:  globally orthotropic with material axes determined by 
vectors. 
TLAT 
HLAT 
Phase change temperature 
Latent heat 
T1 ...  T8 
Temperatures: T1 ...  T8 
C1 ...  C8 
Specific heat at T1 ...  T8 
(K1)1 ...  
(K1)8 
(K2)1 ...  
(K2)8 
(K3)1 ...  
(K3)8 
Thermal conductivity K1 in local x-direction at T1 ...  T8 
Thermal conductivity K2 in local y-direction at T1 ...  T8 
Thermal conductivity K3 in local z-direction at T1 ...  T8 
XP, YP, ZP 
Define coordinate of point  p for AOPT = 1 
A1, A2, A3 
Define components of vector a for AOPT = 2 
D1, D2, D3 
Define components of vector d for AOPT = 2
*MAT_THERMAL_DISCRETE_BEAM 
This  is  thermal  material  type  5.    It  defines  properties  for  discrete  beams.    It  is  only 
applicable when used with *SECTION_BEAM elform = 6. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TMID 
TRO 
Type 
A8 
F 
  Card 2 
Variable 
1 
HC 
Type 
F 
2 
TC 
F 
3 
4 
5 
6 
7 
8 
  VARIABLE   
TMID 
DESCRIPTION
Thermal  material  identification.    A  unique  number  or  label  not
exceeding 8 characters must be specified. 
TRO 
Thermal density: 
EQ.0.0:  default to structural density.   
Specific heat 
Thermal conductance (SI units are W/K) 
  HC   =   (heat transfer coefficient) × (beam cross section area) 
[W/K]   =   [W / m^2 K] * [m^2] 
HC 
TC 
Note: 
A  beam  cross  section  area  is  not  defined  on  the  SECTION_BEAM  keyword  for  an 
elform = 6  discrete  beam.    A  beam  cross  section  area  is  needed  for  heat  transfer 
calculations.  Therefore, the cross section area is lumped into the value entered for HC.
*MAT_THERMAL_CHEMICAL_REACTION 
This is thermal material type 6.  The chemical species making up this material undergo 
chemical reactions.  A maximum of 8 species and 8 chemical reactions can be defined.  
The  thermal  material  properties  of  a  finite  element  undergoing  chemical  reactions  are 
calculated based on a mixture law consisting of those chemical species currently present 
in  the  element.    The  dependence  of  the  chemical  reaction  rate  on  temperature  is 
described by the Arrhenius equation.  Time step splitting is used to couple the system 
of ordinary differential equations describing the chemical reaction kinetics to the system 
of partial differential equations describing the diffusion of heat. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TMID 
NCHSP 
NCHRX 
ICEND 
CEND 
RBEGIN 
GASC 
Type 
A8 
I 
I 
I 
R 
R 
R 
Chemical  Species  Cards.    Include  one  card  for  each  of  the  NCHSP  species.    These 
cards set species properties.  The dummy index i is the species number and is equal to 1 
for the first species card, 2 for the second, and so on. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RHOi 
LCCPi 
LCKi 
N0i 
MWi 
Type 
R 
I 
I 
I 
I 
Reaction Cards.  Include one card for each of the NCHSP species.  Each field contains 
the species’s coefficient for one of the NCHRX chemical reactions.  See card format 3 for 
explanation of the species index i. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RCi1 
RCi2 
RCi3 
RCi4 
RCi5 
RCi6 
RCi7 
RCi8 
Type 
R 
R 
R 
R 
R 
R 
R
Reaction  Rate  Exponent  Cards.    Include  one  card  for  each  of  the  NCHSP  species. 
Each field contains the specie’s rate exponent for one of the NCHRX chemical reactions. 
See card format 3 for explanation of the species index i. 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RXi1 
RXi2 
RXi3 
RXi4 
RXi5 
RXi6 
RXi7 
RXi8 
Type 
R 
R 
R 
R 
R 
R 
R 
R 
Pre-exponential  Factor  Card.    Each  field  contains  the  natural  logarithm  of  its 
corresponding reaction’s pre-exponetial factor. 
  Card 6 
Variable 
1 
Z1 
Type 
R 
2 
Z2 
R 
3 
Z3 
R 
4 
Z4 
R 
5 
Z5 
R 
6 
Z6 
R 
7 
Z7 
R 
8 
Z8 
R 
Activation  Energy  Card.    Each  field  contains  the  activation  energy  value  for  its 
corresponding reaction. 
  Card 7 
Variable 
1 
E1 
Type 
R 
2 
E2 
R 
3 
E3 
R 
4 
E4 
R 
5 
E5 
R 
6 
E6 
R 
7 
E7 
R 
8 
E8 
R 
Heat  of  Reaction  Card.    Each  field  contains  the  heat  of  reaction  value  for  its 
corresponding reaction. 
  Card 8 
Variable 
1 
Q1 
Type 
R 
2 
Q2 
R 
3 
Q3 
R 
4 
Q4 
R 
5 
Q5 
R 
6 
Q6 
R 
7 
Q7 
R 
8 
Q8 
R 
  VARIABLE   
TMID 
3-12 (MAT) 
DESCRIPTION
Thermal  material  identification.    A  unique  number  or  label  not
NCHSP 
Number of chemical species (maximum 8) 
NCHRX 
Number of chemical reactions (maximum 8) 
ICEND 
Species number controlling reaction termination 
RBEGIN 
Chemical  reaction  will  start  when  the  sum  of  the  individual
chemical reaction rates are greater than RBEGIN. 
GASC 
RHOi 
LCCPi 
LCKi 
N0i 
MWi 
RCij 
RXij 
Zj 
Ej 
Qj 
Gas constant: 1.987 cal/(g-mole K), 8314.  J/(kg-mole K) 
Density of the ith species 
Load  curve  ID  specifying  specific  heat  vs.    temperature  for  the ith
species. 
Load  curve  ID  specifying  thermal  conductivity  vs.    temperature
for the ith species 
Initial concentration fraction of the ith species 
Molecular weight of the ith species. 
Reaction  coefficient  for  species  i  in  reaction  j.    Leave  blank  for 
undefined reactions 
Rate  exponent  for  species  i  in  reaction  j.    Leave  blank  for 
undefined reactions. 
Pre-exponential  factor  for  reaction  j.    Enter  the  value  as  ln(Z). 
Leave blank for undefined reactions. 
Activation  energy  for  reaction  j.    Leave  blank  for  undefined 
reactions. 
Heat  of  reaction  for  reaction  j.    Leave  blank  for  undefined 
reactions.
Rate Model for a Single Rection: 
Chemical  reactions  are  usually  expressed  in  chemical  equation  notation;  for  example,  a 
chemical reaction involving two reactants and two products is 
𝑎A + 𝑏B → 𝑔G + ℎH,
(MT6.1)
where A, B, G, and H are chemical species such as NaOH or HCl, and 𝑎, 𝑏, 𝑔, and ℎ are 
integers called stoichiometric numbers, indicating the number of molecules involved in a 
single reaction. 
The rate of reaction is the number of individual reactions per unit time.  Using a stoichiometric 
identity, which is just an accounting relation, the rate of reaction is proportional to the 
rate  of  change  in  the  concentrations  of  the  species  involved  in  the  reaction.    For  the 
chemical reaction in Equation (MT6.1), the relation between concentration and rate, 𝑟, is, 
𝑟 = −
d[A]
d𝑡
= −
d[B]
d𝑡
= +
d[G]
d𝑡
= +
d[H]
d𝑡
,
(MT6.2)
where [X] denotes the concentration of species X, and the sign depends on whether or 
not  the  species  is  an  input,  in  which  case  the  sign  is  negative,  or  a  product,  in  which 
case the sign is positive. 
The Model 
This  thermal  material  model  (T06)  is  built  on  the  assumption  that  the  reaction  rate 
depends on the concentration of the input species according to 
𝑟 = 𝑘(𝑇) ∏[X]𝑝𝑋
 , 
where 𝑋 ranges over all species, and, for each species, the exponent, 𝑝X, is determined 
by  empirical  measurement,  but  may  be  approximated  by  the  stoichiometric  number 
associated with 𝑋.  The proportionality constant, 𝑘, is related to the cross-section for the 
reaction, and it depends on temperature through the Arrhenius equation: 
𝑘 = 𝑍(𝑇) exp (−
𝐸𝑖
𝑅𝑇
), 
where  𝑍(𝑇)  is  experimentally  determined  ,  𝐸𝑖  is  the  activation  energy  ,  𝑅  is  the  gas  constant,  and  𝑇  is  temperature.    As  an  example,  for  the  chemical 
reaction of Equation (MT6.1) 
𝑟 = 𝑍(𝑇) exp (−
𝐸𝑖
𝑅𝑇
) [A]𝛼[B]𝛽, 
where  the  stoichiometric  numbers  have  been  used 
determined exponents. 
instead  of  experimentally
The rate of heat generation (exothermic) and absorption (endothermic) associated with 
a reaction is calculated by multiplying the heat of reaction, 𝑄𝑖 , by its rate. 
Rate Model for a System of Reactions: 
For  a  system  of  coupled  chemical  reactions,  the  change  in  a  species’s  concentration  is 
the sum of all the contributions from each individual chemical reaction: 
d[X]
d𝑡
= ∑(±)𝑖𝑛(𝑥)𝑖𝑟𝑖
. 
The  index i  runs  over all  reactions;  𝑛(𝑥)𝑖  is  the  stoichiometric  number  for  species X  in 
reaction 𝑖; and where 𝑟𝑖 is the rate of reaction 𝑖.  The sign (±)𝑖 is positive for reactions 
that have X as a product and negative for reactions that involve X as an input. 
Example: 
For the following system of reactions 
A → B
A + B → C
2B → C
⇒
⇒
⇒
𝑟1 = 𝑘1[A]
𝑟2 = 𝑘2[A][B]
𝑟3 = 𝑘3[B]2
(MT6.3)
the time evolution equations are, 
d[A]
d𝑡
d[B]
d𝑡
d[C]
d𝑡
= ∑ 𝑛(𝑥)𝑖𝑟𝑖 = −𝑘1[A] − 𝑘2[A][B]
= ∑ 𝑛(𝑥)𝑖𝑟𝑖 = +𝑘1[A] − 𝑘2[A][B] − 2𝑘3[B]2 
(MT6.4)
= ∑ 𝑛(𝑥)𝑖𝑟𝑖 =
+ 𝑘2[A][B] + 𝑘3[B]2.
The coefficients should be identically copied from (MT6.4): 
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RC11 
RC12 
RC13 
RC14 
RC15 
RC16 
RC17 
RC18 
Value 
-1 
-1 
0 
Variable 
RC21 
RC22 
RC23 
RC24 
RC25 
RC26 
RC27 
RC28 
Value 
+1 
-1 
-2
Variable 
RC31 
RC32 
RC33 
RC34 
RC35 
RC36 
RC37 
RC38 
Value 
0 
1 
1 
The exponents are likewise picked off of (MT6.3) for next set of cards in format 5: 
Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RX11 
RX12 
RX13 
RX14 
RX15 
RX16 
RX17 
RX18 
Value 
+1 
+1 
0 
Variable 
RX21 
RX22 
RX23 
RX24 
RX25 
RX26 
RX27 
RX28 
Value 
0 
+1 
+2 
Variable 
RX31 
RX32 
RX33 
RX34 
RX35 
RX36 
RX37 
RX38 
Value 
0 
0 
0 
Equivalent Units (Normalized Units): 
The  concentrations  are  often  scaled  so  that  each  unit  of  reactant  yields  one  unit  of 
product.  Systems for which each species is assigned its own unit of concentration based 
on stoichiometric considerations are equivalent unit systems. 
Being  unit-agnostic,  LS-DYNA  is  capable  of  working  in  equivalent  units.    However, 
care  must  be  taken  so  that  units  are  treated  consistently,  as  applying  a  unit  scaling  to 
the time evolution equations can be nontrivial. 
1.  For  each  reaction,  the  experimentally  measured  pre-exponential  coefficients 
carry units that depend on the reaction itself.  For instance, the pre-exponential 
factors 𝑍1, 𝑍2, and 𝑍3 for the reactions A → B, A + B → C, and 2B → 𝐶 respec-
tively will have units of 
[𝑍1] =
[𝑍2] =
[time]
[time]
×
×
[Concentration of A]
[Concentration of A]
×
[Concentration  of B]
[𝑍3] =
[time]
× {
[Concentration of B]
}
. 
Note that each prefactor has a different dimensionality.
2.  The  equations  in  (MT6.2),  which  relate  rate  to  concentration  change,  are 
logically  inconsistent  unless  all  species  are  measured  using  the  same  units  for 
concentration.    A  species-dependent  system  of  equivalent  units  would  require 
the insertion of additional conversion factors into (MT6.2) thereby changing the 
form of the time-evolution equations. 
To avoid unit consistency issues, it is recommended 
that  reactions  be  defined  in  the  same  unit  system 
that was used to measure their empirical values. 
Example of Equivalent Units: 
The reaction of Equation (MT6.3), 
A → B
A + B → C
2B → C
changes species A into species C through an intermediate which is species B.  For each 
unit of  species C that is produced, the reaction consumes two units of species A.  Since 
this  set  of  chemical  formulae  corresponds  to  the  curing  of  epoxy,  which  is  a  nearly 
volume-preserving process, it is customary to work in a system of equivalent units that 
correspond to species volume fractions. 
The following set of equivalent units, then, is used in the published literature: 
1.  Whatever  the  starting  concentration  of  species  A  is,  all  units  are  uniformly 
rescaled  so  that  [A] = 1  at  time  zero.    Per  the  boxed  remark  above,  since  the 
constants  were  measured  with  respect  to  these  units,  this  consideration  does 
not introduce new complexity. 
2.  Since the process preserves volume, and since one particle of species C replaces 
two particles of species A (and one particle of B replace one of A), the units of 
concentration for species C are doubled. 
𝐶̃ = 2[C] 
Under this transformation the rate relation for C is 
𝑟 = ±
d[C]
d𝑡
=
d𝐶̃
d𝑡
  . 
The time evolution Equations (MT6.4) become, (note [C] has been replaced by 𝐶̃) 
d[A]
d𝑡
= ∑ 𝑛(𝑥)𝑖𝑟𝑖 = −𝑘1[A] − 𝑘2[A][B]
d[B]
d𝑡
d𝐶̃
d𝑡
= ∑ 𝑛(𝑥)𝑖𝑟𝑖 = +𝑘1[A] − 𝑘2[A][B] − 2𝑘3[B]2 
=   ∑ 𝑛(𝑥)𝑖𝑟𝑖 =
+ 2𝑘2[A][B] + 2𝑘3[B]2. 
Whence, 
Therefore, since 
d[A]
d𝑡
+
d[B]
d𝑡
+
d𝐶̃
d𝑡
= 0. 
[A] + [B] + 𝐶̃ = 1 
for all values of time, and since concentration values cannot become negative, it is clear 
that [A], [B], and 𝐶̃ are volume fractions.
*MAT_T07 
This  is  thermal  material  type  7.    It  is  a  thermal  material  with  temperature  dependent 
properties  that  allows  for  material  creation  triggered  by  temperature.    The  acronym 
CWM  stands  for  Computational  Welding  Mechanics  and  the  model  is  intended  to  be 
used  for  simulating  multistage  weld  processes  in  combination  with  the  mechanical 
counterpart, *MAT_CWM. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TMID 
TRO 
TGRLC 
TGMULT 
HDEAD  TDEAD 
Type 
A8 
  Card 2 
1 
F 
2 
F 
3 
F 
4 
F 
5 
F 
6 
7 
8 
Variable 
LCHC 
LCTC 
TLSTART
TLEND 
TISTART 
TIEND 
HGHOST 
TGHOST 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
  VARIABLE   
TMID 
DESCRIPTION
Thermal  material  identification.    A  unique  number  or  label  not
exceeding 8 characters must be specified. 
TRO 
Thermal density: 
EQ.0.0: default to structural density. 
TGRLC 
Thermal generation rate curve number, see *DEFINE_CURVE: 
GT.0:  function versus time, 
EQ.0:  use constant multiplier value, TGMULT, 
LT.0:  function versus temperature. 
TGMULT 
Thermal generation rate multiplier: 
EQ.0.0:  no heat generation. 
HDEAD 
Specific heat for inactive material before birth time 
TDEAD 
Thermal conductivity for inactive material before birth time
LCHC 
*MAT_THERMAL_CWM 
DESCRIPTION
Load curve (or table) for specific heat as function of temperature
(and maximum temperature up to current time)  
LCTC 
Load curve for thermal conductivity as function of temperature 
TLSTART 
Birth temperature of material start 
TLEND 
Birth temperature of material end 
TISTART 
Birth time start 
TIEND 
Birth time end 
HGHOST 
Specific heat for ghost (quiet) material 
TGHOST 
Thermal conductivity for ghost (quiet) material 
Remarks: 
This material is initially in a quiet state, sometimes referred to as a ghost material.  In this 
state  the  material  has  the  thermal  properties  defined  by  the  quiet  specific  heat 
(HGHOST)  and  quiet  thermal  conductivity  (TGHOST).    These  should  represent  the 
void, for example, by picking a relatively small thermal conductivity. 
However, the ghost specific heat must be chosen with care, since the temperature must 
be allowed to increase at a reasonable rate due to the heat from the weld source.  When 
the  temperature  reaches  the  birth  temperature,  a  history  variable  representing  the 
indicator of the welding material is incremented.  This variable follows 
𝛾(𝑡) = min [1, max (0,
𝑇max − 𝑇𝑙
end − 𝑇𝑙
𝑇𝑙
start
start
)] 
where 𝑇max = max{𝑇(𝑠)|𝑠 < 𝑡}. 
The effective thermal material properties are interpolated as 
quiet(1 − 𝛾) 
𝑐 ̃𝑝 = 𝑐𝑝(𝑇, 𝑇max)𝛾 + 𝑐𝑝
𝜇̃ = 𝜇(𝑇)𝛾 + 𝜇quiet(1 − 𝛾) 
where  𝑐𝑝 and  𝜇  are  the  specific  heat  and  thermal  conductivity, respectively.    Here, the 
specific heat, 𝑐𝑝, is either a temperature dependent curve, or a collection of temperature 
dependent curves, ordered in a table according to maximum temperature 𝑇𝑚𝑎𝑥.
The time parameters for creating the material provide additional formulae for the final 
values  of  the  thermal  properties.    Before  the  birth  time  𝑡𝑖
start  of  the  material  has  been 
reached,  the  specific  heat  𝑐𝑝
dead  and  thermal  conductivity  𝜇dead  are  used.    The  default 
values, i.e.  the values used if no user input is given, are  
dead = 1010𝑐𝑝(𝑇, 𝑇max) 
𝑐𝑝
𝜇dead = 0 
Thus, the final values of the thermal properties read 
𝑐𝑝 =
𝜇 =
⎧
{{{{{{
{{{{{{
⎨
⎩
dead
𝑐𝑝
start
𝑡 − 𝑡𝑖
end − 𝑡𝑖
𝑡𝑖
start
dead
+ 𝑐𝑝
end
𝑡 − 𝑡𝑖
start − 𝑡𝑖
𝑡𝑖
end
𝑐 ̃𝑝
𝑐 ̃𝑝
𝜇dead
start
𝑡 − 𝑡𝑖
end − 𝑡𝑖
𝑡𝑖
start
+ 𝜇dead
end
𝑡 − 𝑡𝑖
start − 𝑡𝑖
𝑡𝑖
end
𝜇̃
𝜇̃
⎧
{{{{{{
{{{{{{
⎨
⎩
start
𝑡 ≤ 𝑡𝑖
start < 𝑡 ≤ 𝑡𝑖
𝑡𝑖
end
end < 𝑡
𝑡𝑖
start
𝑡 ≤ 𝑡𝑖
start < 𝑡 ≤ 𝑡𝑖
𝑡𝑖
end
. 
end < 𝑡
𝑡𝑖
These parameters allow the user to control when the welding layor becomes active and 
thereby define a multistage welding process.  Prior to the birth time, the temperature is 
kept  more  or  less  constant  due  to  the  large  specific  heat,  and,  thus,  the  material  is 
prevented from being created
*MAT_THERMAL_ORTHOTROPIC_TD_LC 
This is thermal material type 8.  It allows temperature dependent orthotropic properties 
to be defined by load curves.  The temperature dependency is defined by specifying a 
minimum of two data points.  The properties must be defined for the temperature range 
that the material will see in the analysis. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TMID 
TRO 
TGRLC 
TGMULT 
AOPT 
TLAT 
HLAT 
F 
5 
5 
A2 
F 
5 
F 
6 
6 
A3 
F 
6 
F 
7 
8 
7 
8 
7 
8 
Type 
A8 
  Card 2 
1 
F 
2 
F 
3 
F 
4 
Variable 
LCC 
LCK1 
LCK2 
LCK3 
Type 
I 
I 
I 
I 
4 
A1 
F 
4 
2 
YP 
F 
2 
D2 
F 
3 
ZP 
F 
3 
D3 
F 
  Card 3 
Variable 
1 
XP 
Type 
F 
  Card 4 
Variable 
1 
D1 
Type 
F 
  VARIABLE   
TMID 
DESCRIPTION
Thermal  material  identification.    A  unique  number  or  label  not
exceeding 8 characters must be specified.
VARIABLE   
DESCRIPTION
TRO 
Thermal density: 
EQ.0.0:  default to structural density. 
TGRLC 
Thermal generation rate curve number, see *DEFINE_CURVE: 
GT.0:  function versus time, 
EQ.0:  use constant multiplier value, TGMULT, 
LT.0:  function versus temperature. 
TGMULT 
Thermal generation rate multiplier: 
EQ.0.0:  no heat generation. 
AOPT 
Material  axes  definition:  : 
EQ.0.0:  locally  orthotropic  with  material  axes  by  element
nodes N1, N2 and N4, 
EQ.1.0:  locally orthotropic with material axes determined by a 
point in space and global location of element center, 
EQ.2.0:  globally orthotropic with material axes determined by
TLAT 
HLAT 
LCC 
LCK1 
LCK2 
LCK3 
vectors. 
Phase change temperature 
Latent heat 
Load Curve Specific Heat 
Load Curve Thermal Conductivity K1 in local x-direction 
Load Curve Thermal Conductivity K2 in local y-direction 
Load Curve Thermal Conductivity K3 in local z-direction 
XP, YP, ZP 
Define coordinate of point  p for AOPT = 1 
A1, A2, A3 
Define components of vector a for AOPT = 2 
D1, D2, D3 
Define components of vector d for AOPT = 2
*MAT_THERMAL_ORTHOTROPIC_TD_LC 
See  *MAT_THERMAL_ORTHOTROPIC  keyword  for  a  description  of  the  orthotropic 
axis options, AOPT.
*MAT_THERMAL_ISOTROPIC_PHASE_CHANGE 
This  is  thermal  material  type  9.    It  allows  temperature  dependent  isotropic  properties 
with  phase  change  to  be  defined.    The  latent  heat  of  the  material  is  defined  together 
with  the  solid  and  liquid  temperatures.    The  temperature  dependency  is  defined  by 
specifying  a  minimum  of  two  and  a  maximum  of  eight  data  points.    The  properties 
must be defined for the temperature range that the material will see in the analysis. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TMID 
TRO 
TGRLC 
TGMULT 
Type 
A8 
F 
F 
F 
  Card 2 
Variable 
1 
T1 
Type 
F 
  Card 3 
Variable 
1 
C1 
Type 
F 
  Card 4 
Variable 
1 
K1 
Type 
F 
2 
T2 
F 
2 
C2 
F 
2 
K2 
F 
3 
T3 
F 
3 
C3 
F 
3 
K3 
F 
4 
T4 
F 
4 
C4 
F 
4 
K4 
F 
5 
T5 
F 
5 
C5 
F 
5 
K5 
F 
6 
T6 
F 
6 
C6 
F 
6 
K6 
F 
7 
T7 
F 
7 
C7 
F 
7 
K7 
F 
8 
T8 
F 
8 
C8 
F 
8 
K8
Card 5 
1 
2 
Variable 
SOLT 
LIQT 
Type 
F 
F 
3 
LH 
F 
4 
5 
6 
7 
8 
  VARIABLE   
TMID 
DESCRIPTION
Thermal  material  identification.    A  unique  number  or  label  not
exceeding 8 characters must be specified. 
TRO 
Thermal density: 
EQ.0.0:  default to structural density.   
TGRLC 
Thermal generation rate curve number, see *DEFINE_CURVE: 
GT.0:  function versus time, 
EQ.0: use constant multiplier value, TGMULT, 
LT.0:  function versus temperature. 
TGMULT 
Thermal generation rate multiplier: 
EQ.0.0: no heat generation. 
T1, …, T8 
Temperatures (T1, …, T8) 
C1, …, C8 
Specific heat at T1, …, T8 
K1, …, K8 
Thermal conductivity at T1, …, T8 
Solid temperature, TS (must be < TL) 
Liquid temperature, TL (must be > TS) 
Latent heat 
SOLT 
LIQT 
LH 
Remarks: 
During  phase  change,  that  is  between  the  solid  and  liquid  temperatures,  the  specific 
heat of the material will be enhanced to account for the latent heat as follows:  
𝑐(𝑡) = 𝑚 [1 − cos2𝜋 (
𝑇 − 𝑇𝑆
𝑇𝐿 − 𝑇𝑆
)] ,
𝑇𝑆 < 𝑇 < 𝑇𝐿
where 
𝑇𝐿 = liquid temperature 
𝑇𝑆 = solid temperature 
𝑇 = temperature 
𝑚 = multiplier such that 𝜆 = ∫ 𝐶(𝑇)𝑑𝑇
𝑇𝐿
𝑇𝑆
𝜆 = latent heat 
𝑐 = specific heat
*MAT_THERMAL_ISOTROPIC_TD_LC 
This  is  thermal  material  type  10.    It  allows  isotropic  thermal  properties  that  are 
temperature dependent specified by load curves to be defined.  The properties must be 
defined for the temperature range that the material will see in the analysis. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TMID 
TRO 
TGRLC 
TGMULT 
Type 
A8 
  Card 2 
1 
F 
2 
F 
3 
F 
4 
Variable 
HCLC 
TCLC 
Type 
F 
F 
5 
6 
7 
8 
  VARIABLE   
TMID 
DESCRIPTION
Thermal  material  identification.    A  unique  number  or  label  not
exceeding 8 characters must be specified. 
TRO 
Thermal density: 
EQ.0.0:  default to structural density.   
TGRLC 
Thermal generation rate curve number, see *DEFINE_CURVE: 
GT.0:  function versus time, 
EQ.0: use constant multiplier value, TGMULT, 
LT.0:  function versus temperature. 
TGMULT 
Thermal generation rate multiplier: 
EQ.0.0: no heat generation. 
HCLC 
TCLC 
Load curve ID specifying specific heat vs.  temperature. 
Load curve ID specifying thermal conductivity vs.  temperature.
*MAT_THERMAL_USER_DEFINED 
These  are  Thermal  Material  Types  11 -  15.    The  user  can  supply  his  own  subroutines.  
Please consult Appendix H for more information. 
  Card 1 
1 
Variable 
MID 
2 
RO 
3 
MT 
4 
5 
6 
7 
8 
LMC 
NVH 
AOPT 
IORTHO 
IHVE 
Type 
A8 
F 
F 
F 
F 
F 
F 
F 
Orthotropic Card 1.  Additional card read in when IORTHO = 1. 
  Card 2 
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
3 
ZP 
F 
4 
A1 
F 
5 
A2 
F 
6 
A3 
F 
7 
8 
Orthotropic Card 2.  Additional card read in when IORTHO = 1. 
  Card 3 
Variable 
1 
D1 
Type 
F 
2 
D2 
F 
3 
D3 
F 
4 
5 
6 
7 
8 
Material  Parameter  Cards.    Set  up  to  8  parameters  per  card.    Include  up  to  4  cards. 
This input ends at the next keyword (“*”) card.  
  Card 4 
Variable 
1 
P1 
Type 
F 
2 
P2 
F 
3 
P3 
F 
4 
P4 
F 
5 
P5 
F 
6 
P6 
F 
7 
P7 
F 
8 
P8 
F 
  VARIABLE   
MID 
LS-DYNA R10.0 
DESCRIPTION
Material identification.  A unique number or label not exceeding 8
VARIABLE   
DESCRIPTION
RO 
MT 
LMC 
NVH 
AOPT 
Thermal mass density. 
User material type (11-15 inclusive). 
Length  of  material  constants  array.    LMC  must  not  be  greater
than 32. 
Number of history variables. 
Material  axes  option  of  orthotropic  materials. 
IORTHO = 1.0. 
  Use 
if
EQ.0.0: locally orthotropic with material axes by element nodes
N1, N2 and N4, 
EQ.1.0: locally orthotropic with material axes determined by a
point in space and global location of element center, 
EQ.2.0: globally  orthotropic  with  material  axes  determined  by
vectors. 
LT.0.0:  the  absolute  value  of  AOPT  is  a  coordinate  system  ID
number  (CID  on  *DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM  or  *DEFINE_CO-
ORDINATE_VECTOR).  Available in R3 version of 971 
and later. 
IORTHO 
Set to 1.0 if the material is orthotropic. 
IHVE 
XP - D3 
P1 
⋮ 
Set  to  1.0  to  activate  exchange  of  history  variables  between
mechanical and thermal user material models. 
Material  axes  orientation  of  orthotropic  materials. 
IORTHO = 1.0 
  Use  if
First material parameter. 
⋮  
PLMC 
LMCth material parameter. 
Remarks: 
1.  The IHVE = 1 option makes it possible for a thermal user material subroutine to 
read the history variables of a mechanical user material subroutine defined for 
the same part and vice versa.  If the integration points for the thermal and me-
chanical elements are not coincident then extrapolation/interpolation is used to 
calculate the value when reading history variables. 
2.  Option TITLE is supported 
3. 
*INCLUDE_TRANSFORM:  Transformation  of  units  is  only  supported  for  RO 
field and vectors on card 2 and 3.

Corporate Address 
Livermore Software Technology Corporation 
P.  O.  Box 712 
Livermore, California 94551-0712 
Support Addresses 
Technology 
Software 
Livermore 
Corporation 
7374 Las Positas Road 
Livermore, California 94551 
Tel:  925-449-2500     Fax:  925-449-2507 
Email:  sales@lstc.com 
Website:  www.lstc.com 
Technology 
Software 
Livermore 
Corporation 
1740 West Big Beaver Road 
Suite 100 
Troy, Michigan  48084 
Tel:  248-649-4728     Fax:  248-649-6328 
Disclaimer 
Copyright  ©  1992-2017  Livermore  Software  Technology  Corporation.    All  Rights 
Reserved. 
LS-DYNA®, LS-OPT® and LS-PrePost® are registered trademarks of Livermore Software 
Technology Corporation in the United States.  All other trademarks, product names and 
brand names belong to their respective owners. 
LSTC  reserves  the  right  to  modify  the  material  contained  within  this  manual  without 
prior notice. 
The  information  and  examples  included  herein  are  for  illustrative  purposes  only  and 
are  not  intended  to  be  exhaustive  or  all-inclusive.    LSTC  assumes  no  liability  or 
responsibility whatsoever for any direct or indirect damages or inaccuracies of any type 
or nature that could be deemed to have resulted from the use of this manual. 
Any  reproduction,  in  whole  or  in  part,  of  this  manual  is  prohibited  without  the  prior
Patents 
LSTC products are protected under the following patents: 
US  Patents:  7167816,  7286972,  7308387,  7382367,  7386425,  7386428,  7392163,  7395128, 
7415400,  7428713,  7472602,  7499050,  7516053,  7533577,  7590514,  7613585,  7640146, 
7657394,  7660480,  7664623,  7702490,  7702494,  7945432,  7953578,  7987143,  7996344, 
8050897,  8069017,  8126684,  8150668,  8165856,  8180605,  8190408,  8200458,  8200464, 
8209157,  8271237,  8296109,  8306793,  8374833,  8423327,  8467997,  8489372,  8494819, 
8515714,  8521484,  8577656,  8612186,  8666719,  8744825,  8768660,  8798973,  8898042, 
9020784,  9098657,  9117042,  9135377,  9286422,  9292632,  9405868,  9430594,  9507892, 
9607115. 
Japan Patents: 5090426, 5281057, 5330300, 5373689, 5404516, 5411013, 5411057, 5431133, 
5520553, 5530552, 5589198, 5601961, 5775708, 5792995, 5823170, 6043146, 6043198. 
Patents: 
China 
ZL200910246429.8, 
ZL201010171603.X, 
ZL201010533046.1, 
ZL201110140142.4, 
ZL201210514668.9, 
ZL201210475617.X, ZL201310081855.7. 
ZL200910207380.5, 
ZL201010128222.3, 
ZL201010174074.9, 
ZL201110035253.9, 
ZL201210039535.0, 
ZL201210422902.5, 
ZL200910165817.3, 
ZL201010132510.6, 
ZL201010287263.7, 
ZL201110065789.5, 
ZL201210286459.3, 
ZL201210424131.3, 
ZL200910221325.1, 
ZL201010155066.X, 
ZL201110037461.2, 
ZL201110132394.2, 
ZL201210275406.1, 
ZL201310021716.5,
AES 
AES.    Copyright  ©  2001,  Dr  Brian  Gladman < brg@gladman.uk.net>,  Worcester,  UK.  
All rights reserved. 
LICENSE TERMS 
The free distribution and use of this software in both source and binary form is allowed 
(with or without changes) provided that: 
1.  distributions of this source code include the above copyright notice, this list of 
conditions and the following disclaimer; 
2.  distributions  in  binary  form  include  the  above  copyright  notice,  this  list  of 
conditions  and  the  following  disclaimer  in  the  documentation  and/or  other 
associated materials; 
3. 
the  copyright  holder's  name  is  not  used  to  endorse  products  built  using  this 
software without specific written permission.  
DISCLAIMER 
This software is provided 'as is' with no explicit or implied warranties in respect of any 
properties, including, but not limited to, correctness and fitness for purpose. 
Issue Date: 21/01/2002
INTRODUCTION 
INTRODUCTION 
CHRONOLOGICAL HISTORY 
DYNA3D originated at the Lawrence Livermore National Laboratory [Hallquist 1976].  
The early applications were primarily for the stress analysis of structures subjected to a 
variety  of  impact  loading.    These  applications  required  what  was  then  significant 
computer resources, and the need for a much faster version was immediately obvious.  
Part of the speed problem was related to the inefficient implementation of the element 
technology which was further aggravated by the fact that supercomputers in 1976 were 
much  slower  than  today’s  PC.    Furthermore,  the  primitive  sliding  interface  treatment 
could  only  treat  logically  regular  interfaces  that  are  uncommon  in  most  finite  element 
discretizations  of  complicated  three-dimensional  geometries;  consequently,  defining  a 
suitable mesh for handling contact was often very difficult.  The first version contained 
trusses, membranes, and a choice of solid elements.  The solid elements ranged from a 
one-point  quadrature  eight-noded  element  with  hourglass  control  to  a  twenty-noded 
element with eight integration points.  Due to the high cost of the twenty node solid, the 
zero  energy  modes  related  to  the  reduced  8-point  integration,  and  the  high  frequency 
content  which  drove  the  time  step  size  down,  higher  order  elements  were  all  but 
abandoned  in  later  versions  of  DYNA3D.   A  two-dimensional  version,  DYNA2D,  was 
developed concurrently. 
A new version of DYNA3D was released in 1979 that was programmed to provide near 
optimal speed on the CRAY-1 supercomputers, contained an improved sliding interface 
treatment  that  permitted  triangular  segments  and  was  an  order  of  magnitude  faster 
than the previous contact treatment.  The 1979 version eliminated structural and higher 
order solid elements and some of the material models of the first version.  This version 
also  included  an  optional  element-wise  implementation  of  the  integral  difference 
method developed by Wilkins et al.  [1974].   
The  1981  version  [Hallquist  1981a]  evolved  from  the  1979  version.    Nine  additional 
material models were added to allow a much broader range of problems to be modeled 
including  explosive-structure  and  soil-structure  interactions.    Body  force  loads  were 
implemented for angular velocities and base accelerations.  A link was also established 
from  the  3D  Eulerian  code,  JOY  [Couch,  et.    al.,  1983]  for  studying  the  structural 
response  to  impacts  by  penetrating  projectiles.    An  option  was  provided  for  storing 
element data on disk thereby doubling the capacity of DYNA3D. 
The  1982  version  of  DYNA3D  [Hallquist  1982]  accepted  DYNA2D  [Hallquist  1980] 
material  input  directly.    The  new  organization  was  such  that  equations  of  state  and 
constitutive  models  of  any  complexity  could  be  easily  added.    Complete  vectorization
INTRODUCTION 
of  the  material  models  had  been  nearly  achieved  with  about  a  10  percent  increase  in 
execution speed over the 1981 version. 
In the 1986 version of DYNA3D [Hallquist and Benson 1986], many new features were 
added,  including  beams,  shells,  rigid  bodies,  single  surface  contact,  interface  friction, 
discrete  springs  and  dampers,  optional  hourglass  treatments,  optional  exact  volume 
integration,  and  VAX/  VMS,  IBM,  UNIX,  COS  operating  systems  compatibility,  that 
greatly expanded its range of applications.  DYNA3D thus became the first code to have 
a general single surface contact algorithm. 
In the 1987 version of DYNA3D [Hallquist and Benson 1987] metal forming simulations 
and composite analysis became a reality.  This version included shell thickness changes, 
the Belytschko-Tsay shell element [Belytschko and Tsay, 1981], and dynamic relaxation.  
Also included were non-reflecting boundaries, user specified integration rules for shell 
and beam elements, a layered composite damage model, and single point constraints. 
New  capabilities  added  in  the  1988  DYNA3D  [Hallquist  1988]  version  included  a  cost 
effective  resultant  beam  element,  a  truss  element,  a  C0  triangular  shell,  the  BCIZ 
triangular  shell  [Bazeley  et  al.    1965],  mixing  of  element  formulations  in  calculations, 
composite  failure  modeling  for  solids,  noniterative  plane  stress  plasticity,  contact 
surfaces  with  spot  welds,  tie  break  sliding  surfaces,  beam  surface  contact,  finite 
stonewalls,  stonewall  reaction  forces,  energy  calculations  for  all  elements,  a  crushable 
foam constitutive model, comment cards in the input, and one-dimensional slidelines. 
By  the  end  of  1988  it  was  obvious  that  a  much  more  concentrated  effort  would  be 
required in the development of this software if problems in crashworthiness were to be 
properly  solved;  therefore,  Livermore  Software  Technology  Corporation  was  founded 
to continue the development of DYNA3D as a commercial version called LS-DYNA3D 
which  was later shortened to LS-DYNA.  The 1989 release introduced many enhanced 
capabilities  including  a  one-way  treatment  of  slide  surfaces  with  voids  and  friction; 
cross-sectional forces for structural elements; an optional user specified minimum time 
step  size  for  shell  elements  using  elastic  and  elastoplastic  material  models;  nodal 
accelerations  in  the  time  history  database;  a  compressible  Mooney-Rivlin  material 
model;  a  closed-form  update  shell  plasticity  model;  a  general  rubber  material  model; 
unique  penalty  specifications  for  each  slide  surface;  external  work  tracking;  optional 
time step criterion for 4-node shell elements; and internal element sorting to allow full 
vectorization of right-hand-side force assembly. 
During  the  last  ten  years,  considerable  progress  has  been  made  as  may  be  seen  in  the 
chronology of the developments which follows. 
Capabilities added in 1989-1990: 
•  arbitrary node and element numbers,
INTRODUCTION 
•  fabric model for seat belts and airbags, 
•  composite glass model, 
•  vectorized type 3 contact and single surface contact, 
•  many more I/O options, 
•  all shell materials available for 8 node thick shell, 
•  strain rate dependent plasticity for beams, 
•  fully vectorized iterative plasticity, 
•  interactive graphics on some computers, 
•  nodal damping, 
•  shell thickness taken into account in shell type 3 contact, 
•  shell thinning accounted for in type 3 and type 4 contact, 
•  soft stonewalls, 
•  print suppression option for node and element data, 
•  massless truss elements, rivets – based on equations of rigid body dynamics, 
•  massless beam elements, spot welds – based on equations of rigid body dynam-
ics, 
•  expanded databases with more history variables and integration points, 
•  force limited resultant beam, 
•  rotational spring and dampers, local coordinate systems for discrete elements, 
•  resultant plasticity for C0 triangular element, 
•  energy dissipation calculations for stonewalls, 
•  hourglass energy calculations for solid and shell elements, 
•  viscous and Coulomb friction with arbitrary variation over surface, 
•  distributed loads on beam elements, 
•  Cowper and Symonds strain rate model, 
•  segmented stonewalls, 
•  stonewall Coulomb friction, 
•  stonewall energy dissipation, 
•  airbags (1990), 
•  nodal rigid bodies, 
•  automatic sorting of triangular shells into C0 groups, 
•  mass scaling for quasi static analyses,
INTRODUCTION 
•  user defined subroutines, 
•  warpage checks on shell elements, 
•  thickness consideration in all contact types, 
•  automatic orientation of contact segments, 
•  sliding interface energy dissipation calculations, 
•  nodal force and energy database for applied boundary conditions, 
•  defined stonewall velocity with input energy calculations, 
Capabilities added in 1991-1992: 
•  rigid/deformable material switching, 
•  rigid bodies impacting rigid walls, 
•  strain-rate effects in metallic honeycomb model 26, 
•  shells and beams interfaces included for subsequent component analyses, 
•  external work computed for prescribed displacement/velocity/accelerations, 
•  linear constraint equations, 
•  MPGS database, 
•  MOVIE database, 
•  Slideline interface file, 
•  automated contact input for all input types, 
•  automatic single surface contact without element orientation, 
•  constraint technique for contact, 
•  cut planes for resultant forces, 
•  crushable cellular foams, 
•  urethane foam model with hysteresis, 
•  subcycling, 
•  friction in the contact entities, 
•  strains computed and written for the 8 node thick shells, 
•  “good” 4 node tetrahedron solid element with nodal rotations, 
•  8 node solid element with nodal rotations, 
•  2 × 2 integration for the membrane element, 
•  Belytschko-Schwer integrated beam, 
•  thin-walled Belytschko-Schwer integrated beam,
INTRODUCTION 
•  improved TAURUS database control, 
•  null material for beams to display springs and seatbelts in TAURUS, 
•  parallel implementation on Crays and SGI computers, 
•  coupling to rigid body codes, 
•  seat belt capability. 
Capabilities added in 1993-1994: 
•  Arbitrary Lagrangian Eulerian brick elements, 
•  Belytschko-Wong-Chiang quadrilateral shell element, 
•  Warping stiffness in the Belytschko-Tsay shell element, 
•  Fast Hughes-Liu shell element, 
•  Fully integrated thick shell element, 
•  Discrete 3D beam element, 
•  Generalized dampers, 
•  Cable modeling, 
•  Airbag reference geometry, 
•  Multiple jet model, 
•  Generalized joint stiffnesses, 
•  Enhanced rigid body to rigid body contact, 
•  Orthotropic rigid walls, 
•  Time zero mass scaling, 
•  Coupling with USA (Underwater Shock Analysis), 
•  Layered spot welds with failure based on resultants or plastic strain, 
•  Fillet welds with failure, 
•  Butt welds with failure, 
•  Automatic eroding contact, 
•  Edge-to-edge contact, 
•  Automatic mesh generation with contact entities, 
•  Drawbead modeling, 
•  Shells constrained inside brick elements, 
•  NIKE3D coupling for springback, 
•  Barlat’s anisotropic plasticity,
INTRODUCTION 
•  Superplastic forming option, 
•  Rigid body stoppers, 
•  Keyword input, 
•  Adaptivity, 
•  First MPP (Massively Parallel) version with limited capabilities. 
•  Built in least squares fit for rubber model constitutive constants, 
•  Large hysteresis in hyperelastic foam, 
•  Bilhku/Dubois foam model, 
•  Generalized rubber model, 
Capabilities added in 1995: 
•  Belytschko - Leviathan Shell 
•  Automatic switching between rigid and deformable bodies. 
•  Accuracy  on  SMP  machines  to  give  identical  answers  on  one,  two  or  more 
processors.   
•  Local coordinate systems for cross-section output can be specified. 
•  Null material for shell elements. 
•  Global body force loads now may be applied to a subset of materials. 
•  User defined loading subroutine. 
•  Improved interactive graphics. 
•  New initial velocity options for specifying rotational velocities.   
•  Geometry  changes  after  dynamic  relaxation  can  be  considered  for  initial 
velocities..   
•  Velocities may also be specified by using material or part ID’s. 
•  Improved speed of brick element hourglass force and energy calculations. 
•  Pressure outflow boundary conditions have been added for the ALE options. 
•  More user control for hourglass control constants for shell elements. 
•  Full vectorization in constitutive models for foam, models 57 and 63. 
•  Damage mechanics plasticity model, material 81, 
•  General linear viscoelasticity with 6 term prony series. 
•  Least squares fit for viscoelastic material constants. 
•  Table definitions for strain rate effects in material type 24.
INTRODUCTION 
•  Improved treatment of free flying nodes after element failure. 
•  Automatic  projection  of  nodes  in  CONTACT_TIED  to  eliminate  gaps  in  the 
surface.   
•  More user control over contact defaults. 
•  Improved interpenetration warnings printed in automatic contact. 
•  Flag for using actual shell thickness in single surface contact logic rather than the 
default.   
•  Definition by exempted part ID’s. 
•  Airbag to Airbag venting/segmented airbags are now supported. 
•  Airbag reference geometry speed improvements by using the reference geometry 
for the time step size calculation.   
•  Isotropic airbag material may now be directly for cost efficiency. 
•  Airbag fabric material damping is specified as the ratio of critical damping.   
•  Ability  to  attach  jets  to  the  structure  so  the  airbag,  jets,  and  structure  to  move 
together. 
•  PVM 5.1 Madymo coupling is available. 
•  Meshes are generated within LS-DYNA3D for all standard contact entities. 
•  Joint damping for translational motion.     
•  Angular  displacements,  rates  of  displacements,  damping  forces,  etc.    in  JNT-
FORC file. 
•  Link between LS-NIKE3D to LS-DYNA3D via *INITIAL_STRESS keywords.   
•  Trim curves for metal forming springback. 
•  Sparse equation solver for springback. 
•  Improved mesh generation for IGES and VDA provides a mesh that can directly 
be used to model tooling in metal stamping analyses. 
•  Capabilities added in 1996-1997 in Version 940: 
•  Part/Material ID’s may be specified with 8 digits. 
•  Rigid body motion can be prescribed in a local system fixed to the rigid body. 
•  Nonlinear least squares fit available for the Ogden rubber model. 
•  Least squares fit to the relaxation curves for the viscoelasticity in rubber. 
•  Fu-Chang rate sensitive foam. 
•  6 term Prony series expansion for rate effects in model 57-now 73 
•  Viscoelastic material model 76 implemented for shell elements. 
•  Mechanical threshold stress (MTS) plasticity model for rate effects.
INTRODUCTION 
•  Thermoelastic-plastic material model for Hughes-Liu beam element. 
•  Ramberg-Osgood soil model 
•  Invariant local coordinate systems for shell elements are optional. 
•  Second order accurate stress updates. 
•  Four noded, linear, tetrahedron element. 
•  Co-rotational solid element for foam that can invert without stability problems. 
•  Improved speed in rigid body to rigid body contacts.   
•  Improved searching for the a_3, a_5 and a10 contact types.   
•  Invariant  results  on  shared  memory  parallel  machines  with  the  a_n    contact 
types. 
•  Thickness offsets in type 8 and 9 tie break contact algorithms.   
•  Bucket sort frequency can be controlled by a load curve for airbag applications. 
•  In automatic contact each part ID in the definition may have unique: 
◦  Static coefficient of friction 
◦  Dynamic coefficient of friction 
◦  Exponential decay coefficient 
◦  Viscous friction coefficient 
◦  Optional contact thickness 
◦  Optional thickness scale factor 
◦  Local penalty scale factor 
•  Automatic  beam-to-beam,  shell  edge-to-beam,  shell  edge-to-shell  edge  and 
single surface contact algorithm. 
•  Release criteria may be a multiple of the shell thickness in types a_3, a_5, a10, 13, 
and 26 contact. 
•  Force  transducers  to  obtain  reaction  forces  in  automatic  contact  definitions.  
Defined manually via segments, or automatically via part ID’s. 
•  Searching depth can be defined as a function of time. 
•  Bucket sort frequency can be defined as a function of time. 
•  Interior contact for solid (foam) elements to prevent “negative volumes.” 
•  Locking joint 
•  Temperature dependent heat capacity added to Wang-Nefske inflator models. 
•  Wang  Hybrid  inflator  model  [Wang,  1996]  with  jetting  options  and  bag-to-bag 
venting. 
•  Aspiration included in Wang’s hybrid model [Nusholtz, Wang, Wylie, 1996].
INTRODUCTION 
•  Extended Wang’s hybrid inflator with a quadratic temperature variation for heat 
capacities [Nusholtz, 1996].   
•  Fabric porosity added as part of the airbag constitutive model. 
•  Blockage of vent holes and fabric in contact with structure or itself considered in 
venting with leakage of gas. 
•  Option  to  delay  airbag  liner  with  using  the  reference  geometry  until  the 
reference area is reached. 
•  Birth time for the reference geometry. 
•  Multi-material Euler/ALE fluids,  
◦  2nd order accurate formulations.   
◦  Automatic coupling to shell, brick, or beam elements 
◦  Coupling using LS-DYNA contact options. 
◦  Element with fluid + void and void material 
◦  Element with multi-materials and pressure equilibrium 
•  Nodal inertia tensors. 
•  2D plane stress, plane strain, rigid, and axisymmetric elements 
•  2D plane strain shell element 
•  2D axisymmetric shell element. 
•  Full contact support in 2D, tied, sliding only, penalty and constraint techniques. 
•  Most material types supported for 2D elements. 
•  Interactive remeshing and graphics options available for 2D. 
•  Subsystem definitions for energy and momentum output. 
•  Boundary element method for incompressible fluid dynamics and fluid-structure 
interaction problems. 
Capabilities added during 1997-1998 in Version 950: 
•  Adaptive refinement can be based on tooling curvature with FORMING contact. 
•  The display of drawbeads is now possible since the drawbead data is output into 
the D3PLOT database. 
•  An  adaptive  box  option,  *DEFINE_BOX_ADAPTIVE,  allows  control  over  the 
refinement level and location of elements to be adapted. 
•  A  root  identification  file,  ADAPT.RID, gives  the  parent  element  ID  for  adapted 
elements. 
•  Draw  bead  box  option,  *DEFINE_BOX_DRAWBEAD,  simplifies  drawbead 
input.
INTRODUCTION 
•  The  new  control  option,  CONTROL_IMPLICIT,  activates  an  implicit  solution 
scheme. 
•  2D Arbitrary-Lagrangian-Eulerian elements are available. 
•  2D automatic contact is defined by listing part ID's. 
•  2D  r-adaptivity  for  plane  strain  and  axisymmetric  forging  simulations  is 
available. 
•  2D automatic non-interactive rezoning as in LS-DYNA2D. 
•  2D plane strain and axisymmetric element with 2x2 selective-reduced integration 
are implemented. 
•  Implicit 2D solid and plane strain elements are available. 
•  Implicit 2D contact is available. 
•  The  new  keyword,  *DELETE_CONTACT_2DAUTO,  allows  the  deletion  of  2D 
automatic contact definitions. 
•  The keyword, *LOAD_BEAM is added for pressure boundary conditions on 2D 
elements. 
•  A viscoplastic strain rate option is available for materials: 
◦  *MAT_PLASTIC_KINEMATIC 
◦  *MAT_JOHNSON_COOK 
◦  *MAT_POWER_LAW_PLASTICITY 
◦  *MAT_STRAIN_RATE_DEPENDENT_PLASTICITY 
◦  *MAT_PIECEWISE_LINEAR_PLASTICITY  
◦  *MAT_RATE_SENSITIVE_POWERLAW_PLASTICITY 
◦  *MAT_ZERILLI-ARMSTRONG 
◦  *MAT_PLASTICITY_WITH_DAMAGE 
◦  *MAT_PLASTICITY_COMPRESSION_TENSION  
•  Material  model,  *MAT_Plasticity_with_DAMAGE,  has  a  piecewise 
linear 
damage curve given by a load curve ID. 
•  The  Arruda-Boyce  hyper-viscoelastic  rubber  model  is  available,  see  *MAT_AR-
RUDA_BOYCE. 
•  Transverse-anisotropic-viscoelastic  material 
for  heart 
tissue,  see  *MAT_-
HEART_TISSUE. 
•  Lung hyper-viscoelastic material, see *MAT_LUNG_TISSUE. 
•  Compression/tension  plasticity  model,  see  *MAT_Plasticity_COMPRESSION_-
TENSION.   
•  The  Lund  strain  rate model,  *MAT_STEINBERG_LUND,  is  added  to Steinberg-
Guinan plasticity model.
INTRODUCTION 
•  Rate  sensitive  foam  model,  *MAT_FU_CHANG_FOAM,  has  been  extended  to 
include engineering strain rates, etc. 
•  Model,  *MAT_MODIFIED_Piecewise_Linear_Plasticity,  is  added  for  modeling 
the failure of aluminum. 
•  Material model, *MAT_SPECIAL_ORTHOTROPIC, added for television shadow 
mask problems. 
•  Erosion strain is implemented for material type, *MAT_bamman_damage. 
•  The  equation  of  state,  *EOS_JWLB,  is  available  for  modeling  the  expansion  of 
explosive gases. 
•  The  reference  geometry  option  is  extended  for  foam  and  rubber  materials  and 
can be used for stress initialization, see *INITIAL_FOAM_REFERENCE_GEOM-
ETRY. 
•  A  vehicle  positioning  option  is  available  for  setting  the  initial  orientation  and 
velocities, see *INITIAL_VEHICLE_KINEMATICS. 
•  A  boundary  element  method  is  available  for  incompressible  fluid  dynamics 
problems. 
•  The  thermal  materials  work  with  instantaneous  coefficients  of  thermal  expan-
sion: 
◦  *MAT_ELASTIC_PLASTIC_THERMAL 
◦  *MAT_ORTHOTROPIC_THERMAL 
◦  *MAT_TEMPERATURE_DEPENDENT_ORTHOTROPIC 
◦  *MAT_ELASTIC_WITH_VISCOSITY 
•  Airbag interaction flow rate versus pressure differences. 
•  Contact segment search option, [bricks first optional] 
•  A through thickness Gauss integration rule with 1-10 points is available for shell 
elements.  Previously, 5 were available. 
•  Shell element formulations can be changed in a full deck restart. 
•  The tied interface which is based on constraint equations, TIED_SURFACE_TO_-
SURFACE, can now fail if_FAILURE, is appended. 
•  A general failure criteria for solid elements is independent of the material type, 
see *MAT_ADD_EROSION 
•  Load curve control can be based on thinning and a flow limit diagram, see *DE-
FINE_CURVE_FEEDBACK. 
•  An option to filter the spotweld resultant forces prior to checking for failure has 
been  added  the  the  option,  *CONSTRAINED_SPOTWELD,  by  appending  FIL-
TERED_FORCE, to the keyword.
INTRODUCTION 
•  Bulk viscosity is available for shell types 1, 2, 10, and 16. 
•  When  defining  the  local  coordinate  system  for  the  rigid  body  inertia  tensor  a 
local coordinate system ID can be used.  This simplifies dummy positioning. 
•  Prescribing displacements, velocities, and accelerations is now possible for rigid 
body nodes. 
•  One way flow is optional for segmented airbag interactions. 
•  Pressure time history input for airbag type, LINEAR_FLUID, can be used. 
•  An option is available to independently scale system damping by part ID in each 
of the global directions. 
•  An option is available to independently scale global system damping in each of 
the global directions. 
•  Added option to constrain global DOF along lines parallel with the global axes.  
The keyword is *CONSTRAINED_GLOBAL.  This option is useful for adaptive 
remeshing. 
•  Beam end code releases are available, see *ELEMENT_BEAM. 
•  An  initial  force  can  be  directly  defined  for  the  cable  material,  *MAT_CABLE_-
DISCRETE_BEAM.    The  specification  of  slack  is  not  required  if  this  option  is 
used. 
•  Airbag pop pressure can be activated by accelerometers. 
•  Termination  may  now  be  controlled  by  contact,  via  *TERMINATION_CON-
TACT. 
•  Modified  shell  elements  types  8,  10  and  the  warping  stiffness  option  in  the 
Belytschko-Tsay  shell  to  ensure  orthogonality  with  rigid  body  motions  in  the 
event that the shell is badly warped.  This is optional in the Belytschko-Tsay shell 
and the type 10 shell. 
•  A  one  point  quadrature  brick  element  with  an  exact  hourglass  stiffness  matrix 
has been implemented for implicit and explicit calculations. 
•  Automatic  file  length  determination  for  D3PLOT  binary  database  is  now 
implemented.    This  insures  that  at  least  a  single  state  is  contained  in  each 
D3PLOT file and eliminates the problem with the states being split between files. 
•  The dump files,  which can be very large, can be placed  in another directory by 
specifying 
on the execution line. 
d=/home/user /test/d3dump 
•  A print flag controls the output of data into the MATSUM and RBDOUT files by 
part  ID's.    The  option,  PRINT,  has  been  added  as  an  option  to  the  *PART  key-
word.
INTRODUCTION 
•  Flag has been added to delete material data from the D3THDT file.  See *DATA-
BASE_EXTENT_BINARY  and  column  25  of  the  19th  control  card  in  the  struc-
tured input. 
•  After  dynamic  relaxation  completes,  a  file  is  written  giving  the  displaced  state 
which can be used for stress initialization in later runs. 
Capabilities added during 1998-2000 in Version 960: 
Most  new  capabilities  work  on  both  the  MPP  and  SMP  versions;  however,  the 
capabilities that are implemented for the SMP version only, which were not considered 
critical  for  this  release,  are  flagged  below.    These  SMP  unique  capabilities  are  being 
extended  for  MPP  calculations  and  will  be  available  in  the  near  future.    The  implicit 
capabilities for MPP require the development of a scalable eigenvalue solver, which is 
under development for a later release of LS-DYNA. 
•  Incompressible  flow  solver  is  available.    Structural  coupling  is  not  yet  imple-
mented. 
•  Adaptive mesh coarsening can be done before the implicit springback calculation 
in metal forming applications. 
•  Two-dimensional  adaptivity  can  be  activated  in  both  implicit  and  explicit 
calculations.  (SMP version only) 
•  An internally generated smooth load curve for metal forming tool motion can be 
activated with the keyword: *DEFINE_CURVE_SMOOTH. 
•  Torsional forces can be carried through the deformable spot welds by using the 
contact  type:  *CONTACT_SPOTWELD_WITH_TORSION  (SMP  version  only 
with a high priority for the MPP version if this option proves to be stable.) 
•  Tie  break  automatic  contact  is  now  available  via  the  *CONTACT_AUTOMAT-
IC_…_TIEBREAK  options.    This  option  can  be  used  for  glued  panels.    (SMP 
only) 
•  *CONTACT_RIGID_SURFACE  option  is  now  available  for  modeling  road 
surfaces (SMP version only). 
•  Fixed rigid walls PLANAR and PLANAR_FINITE are represented in the binary 
output file by a single shell element. 
•  Interference fits can be modeled with the INTERFERENCE option in contact. 
•  A layered shell theory is implemented for several constitutive models including 
the composite models to more accurately represent the shear stiffness of laminat-
ed shells. 
•  Damage  mechanics  is  available  to  smooth  the  post-failure  reduction  of  the 
resultant forces in the constitutive model *MAT_SPOTWELD_DAMAGE.
INTRODUCTION 
•  Finite  elastic  strain  isotropic  plasticity  model  is  available  for  solid  elements.  
*MAT_FINITE_ELASTIC_STRAIN_PLASTICITY. 
•  A shape memory alloy material is available: *MAT_SHAPE_MEMORY. 
•  Reference  geometry  for  material,  *MAT_MODIFIED_HONEYCOMB,  can  be  set 
at arbitrary relative volumes or when the time step size reaches a limiting value.  
This option is now available for all element types including the fully integrated 
solid element. 
•  Non  orthogonal  material  axes  are  available  in  the  airbag  fabric  model.    See 
*MAT_FABRIC. 
•  Other new constitutive models include for the beam elements: 
◦  *MAT_MODIFIED_FORCE_LIMITED 
◦  *MAT_SEISMIC_BEAM 
◦  *MAT_CONCRETE_BEAM 
•  for shell and solid elements: 
◦  *MAT_ELASTIC_VISCOPLASTIC_THERMAL 
•  for the shell elements: 
◦  *MAT_GURSON 
◦  *MAT_GEPLASTIC_SRATE2000 
◦  *MAT_ELASTIC_VISCOPLASTIC_THERMAL 
◦  *MAT_COMPOSITE_LAYUP 
◦  *MAT_COMPOSITE_LAYUP 
◦  *MAT_COMPOSITE_DIRECT  
•  for the solid elements: 
◦  *MAT_JOHNSON_HOLMQUIST_CERAMICS 
◦  *MAT_JOHNSON_HOLMQUIST_CONCRETE 
◦  *MAT_INV_HYPERBOLIC_SIN 
◦  *MAT_UNIFIED_CREEP 
◦  *MAT_SOIL_BRICK 
◦  *MAT_DRUCKER_PRAGER 
◦  *MAT_RC_SHEAR_WALL 
•  and for all element options a very fast and efficient version of the Johnson-Cook 
plasticity model is available: 
•  *MAT_SIMPLIFIED_JOHNSON_COOK  
•  A  fully  integrated  version  of  the  type  16  shell  element  is  available  for  the 
resultant constitutive models.
INTRODUCTION 
•  A  nonlocal  failure  theory  is  implemented  for  predicting  failure  in  metallic 
materials.  The keyword *MAT_NONLOCAL activates this option for a subset of 
elastoplastic constitutive models. 
•  A  discrete  Kirchhoff  triangular  shell  element  (DKT)  for  explicit  analysis  with 
three  in  plane  integration  points  is  flagged  as  a  type  17  shell  element.    This 
element has much better bending behavior than the C0 triangular element. 
•  A discrete Kirchhoff linear triangular and quadrilateral shell element is available 
as a type 18 shell.  This shell is for extracting normal modes and static analysis. 
•  A C0 linear 4-node quadrilateral shell element is implemented as element type 20 
with drilling stiffness for normal modes and static analysis. 
•  An assumed strain linear brick element is available for normal modes and statics. 
•  The  fully  integrated  thick  shell  element  has  been  extended  for  use  in  implicit 
calculations. 
•  A fully integrated thick shell element based on an assumed strain formulation is 
now available.  This element uses a full 3D constitutive model which includes the 
normal  stress  component  and,  therefore,  does  not  use  the  plane  stress  assump-
tion. 
•  The  4-node  constant  strain  tetrahedron  element  has  been  extended  for  use  in 
implicit calculations. 
•  Relative damping between parts is available, see *DAMPING_RELATIVE (SMP 
only).   
•  Preload forces are can be input for the discrete beam elements. 
•  Objective  stress  updates  are  implemented  for  the  fully  integrated  brick  shell 
element. 
•  Acceleration time histories can be prescribed for rigid bodies. 
•  Prescribed motion for nodal rigid bodies is now possible. 
•  Generalized  set  definitions,  i.e.,  SET_SHELL_GENERAL  etc.    provide  much 
flexibility in the set definitions. 
•  The command “sw4.” will write a state into the dynamic relaxation file, D3DRLF, 
during the dynamic relaxation phase if the D3DRLF file is requested in the input. 
•  Added mass by PART ID is written into the MATSUM file when mass scaling is 
used to maintain the time step size, (SMP version only). 
•  Upon termination due to a large mass increase during a mass scaled calculation a 
print summary of 20 nodes with the maximum added mass is printed. 
•  Eigenvalue  analysis  of  models  containing  rigid  bodies  is  now  available  using 
BCSLIB-EXT solvers from Boeing.  (SMP version only).
INTRODUCTION 
•  Second  order  stress  updates  can  be  activated  by  part  ID  instead  of  globally  on 
the *CONTROL_ACCURACY input. 
•  Interface  frictional  energy  is  optionally  computed  for  heat  generation  and  is 
output into the interface force file (SMP version only). 
•  The  interface  force  binary  database  now  includes  the  distance  from  the  contact 
surface for the FORMING contact options.  This distance is given after the nodes 
are detected as possible contact candidates.  (SMP version only). 
•  Type 14 acoustic brick element is implemented.  This element is a fully integrat-
ed version of type 8, the acoustic element (SMP version only). 
•  A  flooded  surface  option  for  acoustic  applications  is  available  (SMP  version 
only). 
•  Attachment nodes can be defined for rigid bodies.  This option is useful for NVH 
applications. 
•  CONSTRAINED_POINTS tie any two points together.  These points must lie on 
a shell elements. 
•  Soft constraint is available for edge to edge contact in type 26 contact. 
•  CONSTAINED_INTERPOLATION  option  for  beam  to  solid  interfaces  and  for 
spreading the mass and loads.  (SMP version only). 
•  A database option has been added that allows the output of added mass for shell 
elements instead of the time step size. 
•  A  new  contact  option  allows  the  inclusion  of  all  internal  shell  edges  in  contact 
type *CONTACT_GENERAL, type 26.  This option is activated by adding “_IN-
TERIOR” after the GENERAL keyword. 
•  A  new  option  allows  the  use  deviatoric  strain  rates  rather  than  total  rates  in 
material model 24 for the Cowper-Symonds rate model. 
•  The  CADFEM  option  for  ASCII  databases  is  now  the  default.    Their  option 
includes more significant figures in the output files. 
•  When  using  deformable  spot  welds,  the  added  mass  for  spot  welds  is  now 
printed for the case where global mass scaling is activated.  This output is in the 
log file, d3hsp file, and the messag file. 
•  Initial  penetration  warnings  for  edge-to-edge  contact  are  now  written  into  the 
MESSAG file and the d3hsp file. 
•  Each compilation of LS-DYNA is given a unique version number. 
•  Finite length discrete beams with various local axes options are now available for 
material types 66, 67, 68, 93, and 95.  In this implementation the absolute value of 
SCOOR must be set to 2 or 3 in the *SECTION_BEAM input. 
•  New discrete element constitutive models are available:
INTRODUCTION 
◦  *MAT_ELASTIC_SPRING_DISCRETE_BEAM 
◦  *MAT_INELASTIC_SPRING_DISCRETE_BEAM 
◦  *MAT_ELASTIC_6DOF_SPRING_DISCRETE_BEAM 
◦  *MAT_INELASTIC_6DOF_SPRING_DISCRETE_BEAM 
•  The latter two can be used as finite length beams with local coordinate systems. 
•  Moving  SPC's  are  optional  in  that  the  constraints  are  applied  in  a  local  system 
that rotates with the 3 defining nodes. 
•  A moving local coordinate system, CID, can be used to determine orientation of 
discrete beam elements.   
•  Modal  superposition  analysis  can  be  performed  after  an  eigenvalue  analysis.  
Stress recovery is based on type 18 shell and brick (SMP only). 
•  Rayleigh damping input factor is now input as a fraction of critical damping, i.e.  
0.10.    The  old  method  required  the  frequency  of  interest  and  could  be  highly 
unstable for large input values. 
•  Airbag  option  “SIMPLE_PRESSURE_VOLUME”  allows  for  the  constant  CN  to 
be  replaced  by  a  load  curve  for  initialization.    Also,  another  load  curve  can  be 
defined  which  allows  CN  to  vary  as  a  function  of  time  during  dynamic  relaxa-
tion.  After dynamic relaxation CN can be used as a fixed constant or load curve. 
•  Hybrid inflator model utilizing CHEMKIN and NIST databases is now available.  
Up to ten gases can be mixed. 
•  Option to track initial penetrations has been added in the automatic SMP contact 
types  rather  than  moving  the  nodes  back  to  the  surface.    This  option  has  been 
available  in  the  MPP  contact  for  some  time.    This  input  can  be  defined  on  the 
fourth card of the *CONTROL_CONTACT input and on each contact definition 
on the third optional card in the *CONTACT definitions. 
•  If the average acceleration flag is active, the average acceleration for rigid body 
nodes is now written into the D3THDT and NODOUT files.  In previous versions 
of LS-DYNA, the accelerations on rigid nodes were not averaged. 
•  A  capability  to  initialize  the  thickness  and  plastic  strain  in  the  crash  model  is 
available  through  the  option  *INCLUDE_STAMPED_PART,  which  takes  the 
results  from  the  LS-DYNA  stamping  simulation  and  maps  the  thickness  and 
strain distribution onto the same part with a different mesh pattern. 
•  A  capability  to  include  finite  element  data  from  other  models  is  available 
through the option, *INCLUDE_TRANSFORM.  This option will take the model 
defined in an INCLUDE file: offset all ID's; translate, rotate, and scale the coordi-
nates; and transform the constitutive constants to another set of units.
INTRODUCTION 
Features added during 2001-2002 for the 970 release of LS-DYNA: 
Some of the new features, which are also listed below, were also added to later releases 
of version 960.  Most new explicit capabilities work for both the MPP and SMP versions; 
however,  the  implicit  capabilities  for  MPP  require  the  development  of  a  scalable 
eigenvalue  solver  and  a  parallel  implementation  of  the  constraint  equations  into  the 
global matrices.   This work is underway.  A later release of version 970 is planned in 
2003 that will be scalable for implicit solutions. 
Below is list of new capabilities and features: 
•  MPP  decomposition  can  be  controlled  using  *CONTROL_MPP_DECOMPOSI-
TION commands in the input deck. 
•  The  MPP  arbitrary  Lagrangian-Eulerian  fluid  capability  now  works  for  airbag 
deployment in both SMP and MPP calculations. 
•  Euler-to-Euler  coupling 
is  now  available  through  the  keyword  *CON-
STRAINED_EULER_TO_EULER. 
•  Up  to  ten  ALE  multi-material  groups  may  now  be  defined.    The  previous  limit 
was three groups. 
•  Volume  fractions  can  be  automatically  assigned  during  initialization  of  multi-
material cells.  See the GEOMETRY option of *INITIAL_VOLUME_FRACTION. 
•  A new ALE smoothing option is available to accurately predict shock fronts. 
•  DATABASE_FSI activates output of fluid-structure interaction data to ASCII file 
DBFSI. 
•  Point sources for airbag inflators are available.  The origin and mass flow vector 
of these inflators are permitted to vary with time. 
•  A  majority  of  the  material  models  for  solid  materials  are  available  for  calcula-
tions using the SPH (Smooth Particle Hydrodynamics) option.   
•  The  Element  Free  Galerkin  method  (EFG  or  meshfree)  is  available  for  two-
dimensional  and  three-dimensional  solids.    This  new  capability  is  not  yet  im-
plemented for MPP applications. 
•  A  binary  option  for  the  ASCII  files  is  now  available.    This  option  applies  to  all 
ASCII files and results in one binary file that contains all the information normal-
ly spread between a large number of separate ASCII files. 
•  Material models can now be defined by numbers rather than long names in the 
keyword  input.   For  example  the  keyword  *MAT_PIECEWISE_LINEAR_PLAS-
TICITY can be replaced by the keyword: *MAT_024. 
•  An  embedded  NASTRAN  reader  for  direct  reading  of  NASTRAN  input  files  is 
available.  This option allows a typical input file for NASTRAN to be read direct-
ly and used without additional input.  See the *INCLUDE_NASTRAN keyword.
INTRODUCTION 
•  Names in the keyword input can represent numbers if the *PARAMETER option 
is used to relate the names and the corresponding numbers.   
•  Model  documentation  for  the  major  ASCII  output  files  is  now  optional.    This 
option allows descriptors to be included within the ASCII files that document the 
contents of the file. 
•  ID’s have been added to the following keywords: 
◦  *BOUNDARY_PRESCRIBED_MOTION 
◦  *BOUNDARY_PRESCRIBED_SPC 
◦  *CONSTRAINED_GENERALIZED_WELD 
◦  *CONSTRAINED_JOINT 
◦  *CONSTRAINED_NODE_SET 
◦  *CONSTRAINED_RIVET 
◦  *CONSTRAINED_SPOTWELD 
◦  *DATABASE_CROSS_SECTION 
◦  *ELEMENT_MASS 
•  Penetration  warnings  for  the  contact  option,  ignore  initial  penetration,  î  are 
added as an option.  Previously, no penetration warnings were written when this 
contact option was activated. 
•  Penetration  warnings  for  nodes  in-plane  with  shell  mid-surface  are  printed  for 
the AUTOMATIC contact options.  Previously, these nodes were ignored since it 
was assumed that they belonged to a tied interface where an offset was not used; 
consequently, they should not be treated in contact. 
•  For  the  arbitrary  spot  weld  option,  the  spot  welded  nodes  and  their  contact 
segments  are  optionally  written  into  the  d3hsp  file.    See  *CONTROL_CON-
TACT. 
•  For  the  arbitrary  spot  weld  option,  if  a  segment  cannot  be  found  for  the  spot 
welded  node,  an  option  now  exists  to  error  terminate.    See  *CONTROL_CON-
TACT. 
•  Spot  weld  resultant  forces  are  written  into  the  SWFORC  file  for  solid  elements 
used as spot welds. 
•  Solid materials have now been added to the failed element report. 
•  A  new  option  for  terminating  a  calculation  is  available,  *TERMINATION_-
CURVE. 
•  A  10-noded  tetrahedron  solid  element  is  available  with  either  a  4  or  5  point 
integration rule.  This element can also be used for implicit solutions. 
•  A  new  4  node  linear  shell  element  is  available  that  is  based  on  Wilson’s  plate 
element combined with a Pian-Sumihara membrane element.  This is shell type 
21.
INTRODUCTION 
•  A shear panel element has been added for linear applications.  This is shell type 
22.  This element can also be used for implicit solutions. 
•  A  null  beam  element  for  visualization  is  available.    The  keyword  to  define  this 
null  beam  is  *ELEMENT_PLOTEL.    This  element  is  necessary  for  compatibility 
with NASTRAN. 
•  A  scalar  node  can  be  defined  for  spring-mass  systems.    The  keyword  to  define 
this node is *NODE_SCALAR.  This node can have from 1 to 6 scalar degrees-of-
freedom. 
•  A  thermal  shell  has  been  added  for  through-thickness  heat  conduction.  
Internally,  8  additional  nodes  are  created,  four  above  and  four  below  the  mid-
surface of the shell element.  A quadratic temperature field is modeled through 
the shell thickness.  Internally, the thermal shell is a 12 node solid element. 
•  A  beam  OFFSET  option  is  available  for  the  *ELEMENT_BEAM  definition  to 
permit  the  beam  to  be  offset  from  its  defining  nodal  points.    This  has  the  ad-
vantage that all beam formulations can now be used as shell stiffeners. 
•  A beam ORIENTATION option for orienting the beams by a vector instead of the 
third  node  is  available  in  the  *ELEMENT_BEAM  definition  for  NASTRAN 
compatibility.   
•  Non-structural  mass  has  been  added  to  beam  elements  for  modeling  trim  mass 
and for NASTRAN compatibility. 
•  An  optional  checking  of  shell  elements  to  avoid  abnormal  terminations  is 
available.  See *CONTROL_SHELL.  If this option is active, every shell is checked 
each  time  step  to  see  if  the  distortion  is  so  large  that  the  element  will  invert, 
which will result in an abnormal termination.  If a bad shell is detected, either the 
shell will be deleted or the calculation will terminate.  The latter is controlled by 
the input. 
•  An  offset  option  is  added  to  the  inertia  definition.   See  *ELEMENT_INERTIA_-
OFFSET  keyword.    This  allows  the  inertia  tensor  to  be  offset  from  the  nodal 
point. 
•  Plastic  strain  and  thickness  initialization  is  added  to  the  draw  bead  contact 
option.  See *CONTACT_DRAWBEAD_INITIALIZE. 
•  Tied contact with offsets based on both constraint equations and beam elements 
for solid elements and shell elements that  have 3 and 6 degrees-of-freedom per 
node,  respectively.    See  BEAM_OFFSET  and  CONSTRAINED_OFFSET  contact 
options.  These options will not cause problems for rigid body motions. 
•  The  segment-based  (SOFT = 2)  contact  is  implemented  for  MPP  calculations.  
This enables airbags to be easily deployed on the MPP version. 
•  Improvements  are  made  to  segment-based  contact  for  edge-to-edge  and  sliding 
conditions, and for contact conditions involving warped segments.
INTRODUCTION 
•  An  improved  interior  contact  has  been  implemented  to  handle  large  shear 
deformations in the solid elements.  A special interior contact algorithm is avail-
able for tetrahedron elements. 
•  Coupling with MADYMO 6.0 uses an extended coupling that allows users to link 
most  MADYMO  geometric  entities  with  LS-DYNA  FEM  simulations.    In  this 
coupling  MADYMO  contact  algorithms  are  used  to  calculate  interface  forces 
between the two models. 
•  Release  flags  for  degrees-of-freedom  for  nodal  points  within  nodal  rigid  bodies 
are  available.    This  makes  the  nodal  rigid  body  option  nearly  compatible  with 
the RBE2 option in NASTRAN. 
•  Fast  updates  of  rigid  bodies  for  metalforming  applications  can  now  be  accom-
plished by ignoring the rotational degrees-of-freedom in the rigid bodies that are 
typically  inactive  during  sheet  metal  stamping  simulations.    See  the  keyword: 
*CONTROL_RIGID. 
•  Center  of  mass  constraints  can  be  imposed  on  nodal  rigid  bodies  with  the  SPC 
option in either a local or a global coordinate system. 
•  Joint failure based on resultant forces and moments can now be used to simulate 
the failure of joints. 
•  CONSTRAINED_JOINT_STIFFNESS  now  has  a  TRANSLATIONAL  option  for 
the translational and cylindrical joints. 
•  Joint  friction  has  been  added  using  table  look-up  so  that  the  frictional  moment 
can now be a function of the resultant translational force. 
•  The  nodal  constraint  options  *CONSTRAINED_INTERPOLATION  and  *CON-
STRAINED_LINEAR  now  have  a  local  option  to  allow  these  constraints  to  be 
applied in a local coordinate system. 
•  Mesh  coarsening  can  now  be  applied  to  automotive  crash  models  at  the 
beginning  of  an  analysis  to  reduce  computation  times.    See  the  new  keyword: 
*CONTROL_COARSEN. 
•  Force versus time seatbelt pretensioner option has been added. 
•  Both  static  and  dynamic  coefficients  of  friction  are  available  for  seat  belt  slip 
rings.  Previously, only one friction constant could be defined. 
•  *MAT_SPOTWELD now includes a new failure model with rate effects as well as 
additional failure options. 
•  Constitutive models added for the discrete beam elements: 
◦  *MAT_1DOF_GENERALIZED_SPRING 
◦  *MAT_GENERAL_NONLINEAR_6dof_DISCRETE_BEAM  
◦  *MAT_GENERAL_NONLINEAR_1dof_DISCRETE_BEAM  
◦  *MAT_GENERAL_SPRING_DISCRETE_BEAM
INTRODUCTION 
◦  *MAT_GENERAL_JOINT_DISCRETE_BEAM 
◦  *MAT_SEISMIC_ISOLATOR 
•  for shell and solid elements: 
◦  *MAT_plasticity_with_damage_ortho 
◦  *MAT_simplified_johnson_cook_orthotropic_damage 
◦  *MAT_HILL_3R  
◦  *MAT_GURSON_RCDC 
•  for the solid elements: 
◦  *MAT_SPOTWELD 
◦  *MAT_HILL_FOAM 
◦  *MAT_WOOD 
◦  *MAT_VISCOELASTIC_HILL_FOAM 
◦  *MAT_LOW_DENSITY_SYNTHETIC_FOAM 
◦  *MAT_RATE_SENSITIVE_POLYMER 
◦  *MAT_QUASILINEAR VISCOELASTIC 
◦  *MAT_TRANSVERSELY_ANISOTROPIC_CRUSHABLE_FOAM 
◦  *MAT_VACUUM  
◦  *MAT_MODIFIED_CRUSHABLE_FOAM 
◦  *MAT_PITZER_CRUSHABLE FOAM 
◦  *MAT_JOINTED_ROCK 
◦  *MAT_SIMPLIFIED_RUBBER 
◦  *MAT_FHWA_SOIL 
◦  *MAT_SCHWER_MURRAY_CAP_MODEL 
•  Failure time added to MAT_EROSION for solid elements. 
•  Damping  in  the  material  models  *MAT_LOW_DENSITY_FOAM  and  *MAT_-
LOW_DENSITY_VISCOUS_FOAM  can  now  be  a  tabulated  function  of  the 
smallest stretch ratio. 
•  The  material  model  *MAT_PLASTICITY_WITH_DAMAGE  allows  the  table 
definitions for strain rate. 
•  Improvements in the option *INCLUDE_STAMPED_PART now allow all history 
data  to  be  mapped  to  the  crash  part  from  the  stamped  part.    Also,  symmetry 
planes can be used to allow the use of a single stamping to initialize symmetric 
parts. 
•  Extensive  improvements  in  trimming  result  in  much  better  elements  after  the 
trimming is completed.  Also, trimming can be defined in either a local or global 
coordinate system.  This is a new option in *DEFINE_CURVE_TRIM. 
•  An option to move parts close before solving the contact problem is available, see 
*CONTACT_AUTO_MOVE.
INTRODUCTION 
•  An option to add or remove discrete beams during a calculation is available with 
the new keyword: *PART_SENSOR. 
•  Multiple  jetting  is  now  available  for  the  Hybrid  and  Chemkin  airbag  inflator 
models. 
•  Nearly all constraint types are now handled for implicit solutions. 
•  Calculation of constraint and attachment modes can be easily done by using the 
option: *CONTROL_IMPLICIT_MODES. 
•  Penalty  option,  see  *CONTROL_CONTACT,  now  applies  to  all  *RIGIDWALL 
options and is always used when solving implicit problems. 
•  Solid  elements  types  3  and  4,  the  4  and  8  node  elements  with  6  degrees-of-
freedom per node are available for implicit solutions. 
•  The  warping  stiffness  option  for  the  Belytschko-Tsay  shell  is  implemented  for 
implicit  solutions.    The  Belytschko-Wong-Chang  shell  element  is  now  available 
for  implicit  applications.    The  full  projection  method  is  implemented  due  to  it 
accuracy over the drill projection. 
•  Rigid to deformable switching is implemented for implicit solutions. 
•  Automatic  switching  can  be  used  to  switch  between  implicit  and  explicit 
calculations.  See the keyword: *CONTROL_IMPLICIT_GENERAL. 
•  Implicit dynamics rigid bodies are now implemented.  See the keyword  *CON-
TROL_IMPLICIT_DYNAMIC. 
•  Eigenvalue solutions can be intermittently calculated during a transient analysis. 
•  A  linear  buckling  option  is  implemented.    See  the  new  control  input:  *CON-
TROL_IMPLICIT_BUCKLE 
•  Implicit  initialization  can  be  used  instead  of  dynamic  relaxation.    See  the 
keyword *CONTROL_DYNAMIC_RELAXATION where the parameter, IDFLG, 
is set to 5. 
•  Superelements,  i.e.,  *ELEMENT_DIRECT_MATRIX_INPUT,  are  now  available 
for implicit applications. 
•  There is an extension of the option, *BOUNDARY_CYCLIC, to symmetry planes 
in  the  global  Cartesian  system.    Also,  automatic  sorting  of  nodes  on  symmetry 
planes is now done by LS-DYNA. 
•  Modeling  of  wheel-rail  contact  for  railway  applications  is  now  available,  see 
*RAIL_TRACK and *RAIL_TRAIN. 
•  A  new,  reduced  CPU,  element  formulation  is  available  for  vibration  studies 
when elements are aligned with the global coordinate system.  See *SECTION_-
SOLID and *SECTION_SHELL formulation 98. 
•  An option to provide approximately constant damping over a range of frequen-
cies is implemented, see *DAMPING_FREQUENCY_RANGE.
INTRODUCTION 
Features added during 2003-2005 for the 971 release of LS-DYNA: 
fully 
functional 
Initially,  the  intent  was  to  quickly  release  version  971  after  970  with  the  implicit 
for  distributed  memory  processing  using  MPI.  
capabilities 
Unfortunately, the effort required for parallel implicit was grossly underestimated, and, 
as a result, the release has been delayed.  Because of the delay, version 971 has turned 
into a major release.   Some of the new features, listed below, were also added to later 
releases  of  version  970.    The  new  explicit  capabilities  are  implemented  in  the  MPP 
version and except for one case, in the SMP version as well. 
Below is list of new capabilities and features:  
•  A simplified method for using the ALE capability with airbags is now available 
with the keyword *AIRBAG_ALE. 
•  Case  control  using  the  *CASE  keyword,  which  provides  a  way  of  running 
multiple load cases sequentially within a single run 
•  New  option  to  forming  contact:  *CONTACT_FORMING_ONE_WAY_SUR-
FACE_TO_SURFACE_SMOOTH, which use fitted surface in contact calculation. 
•  Butt weld definition by using the *CONSTRAINED_BUTT_WELD option which 
makes  the  definition  of  butt  welds  simple  relative  to  the  option:  *CON-
STRAINED_GENERALIZED_WELD_BUTT. 
•  H-adaptive  fusion  is  now  possible  as  an  option  with  the  control  input,  *CON-
TROL_ADAPTIVE. 
•  Added  a  parameter  on,  *CONTROL_ADAPTIVE,  to  specify  the  number  of 
elements generated around a 90 degree radius.  A new option to better calculate 
the curvature was also implemented. 
•  Added a new keyword: *CONTROL_ADAPTIVE_CURVE, to refine the element 
along trimming curves 
•  Birth  and  death  times  for  implicit  dynamics  on  the  keyword  *CONTROL_IM-
PLICIT_DYNAMICS. 
•  Added  an  option  to  scale  the  spot  weld  failure  resultants  to  account  for  the 
location  of  the  weld  on  the  segment  surface,  see  *CONTROL_SPOTWELD_-
BEAM. 
•  Added  an  option  which  automatically  replaces  a  single  beam  spot  weld  by  an 
assembly of solid elements using the same ID as the beam that was replaced, see 
*CONTROL_SPOTWELD_BEAM. 
•  Boundary  constraint  in  a  local  coordinate  system  using  *CONSTRAINED_LO-
CAL keyword. 
•  A  cubic  spline  interpolation  element  is  now  available,  *CONSTRAINED_-
SPLINE.
INTRODUCTION 
•  Static implicit analyses in of a structure with rigid body modes is possible using 
the option, *CONTROL_IMPLICIT_INERTIA_RELIEF. 
•  Shell  element  thickness  updates  can  now  be  limited  to  part  ID’s  within  a 
specified set ID, see the *CONTROL_SHELL keyword.  The thickness update for 
shells  can  now  be  optionally  limited  to  the  plastic  part  of  the  strain  tensor  for 
better stability in crash analysis. 
•  Solid  element  stresses  in  spot  welds  are  optionally  output  in  the  local  system 
using the SWLOCL parameter on the *CONTROL_SOLID keyword. 
•  SPOTHIN  option  on  the  *CONTROL_CONTACT  keyword  cards  locally  thins 
the spot welded parts to prevent premature breakage of the weld by the contact 
treatments. 
•  New  function:  *CONTROL_FORMING_PROJECT,  which  can  initial  move  the 
penetrating slave nodes to the master surface 
•  New function *CONTROL_FORMING_TEMPLATE, which allows user to easily 
set up input deck.  Its function includes auto-position, define travel curve, termi-
nation time, and most of the forming parameters for most of the typical forming 
process. 
•  New  function  *CONTROL_FORMING_USER,  *CONTROL_FORMING_POSI-
TION,  and  *CONTROL_FORMING_TRAVEL,  when  used  together,  can  allow 
the user to define atypical forming process. 
•  Added new contact type *CONTACT_GUIDED_CABLE. 
•  Circular cut planes are available for *DATABASE_CROSS_SECTION definitions. 
•  New binary database FSIFOR for fluid structure coupling. 
•  Added  *DATABASE_BINARY_D3PROP  for  writing  the  material  and  property 
data to the first D3PLOT file or to a new database D3PROP. 
•  DATABASE_EXTENT_BINARY  has  new  flags  to  output  peak  pressure,  surface 
energy  density,  nodal  mass  increase  from  mass  scaling,  thermal  fluxes,  and 
temperatures at the outer surfaces of the thermal shell. 
•  Eight-character alphanumeric labels can now be used for the parameters SECID, 
MID, EOSID, HGID, and TMID on the *PART keyword. 
•  Two  NODOUT  files  are  now  written:  one  for  high  frequency  output  and  a 
second for low frequency output. 
•  Nodal  mass  scaling  information  can  now  be  optionally  written  to  the  D3PLOT 
file. 
•  Added option, MASS_PROPERTIES, to include the mass and inertial properties 
in the GLSTAT and SSSTAT files. 
•  Added option in *CONTROL_CPU to output the cpu and elapsed time into the 
GLSTAT file.
INTRODUCTION 
•  Added  an  option,  IERODE,  on  the  *CONTROL_OUTPUT  keyword  to  include 
eroded energies by part ID into the MATSUM file.  Lumped mass kinetic energy 
is also in the MATSUM file as part ID 0.   
•  Added  an  option,  TET10,  on  the  *CONTROL_OUTPUT  keyword  to  output  ten 
connectivity nodes into D3PLOT database rather than 4. 
•  New  keyword,  *ELEMENT_SOLID_T4TOT10  to  convert  4  node  tetrahedron 
elements to 10 node tetrahedron elements. 
•  New  keyword,  *ELEMENT_MASS_PART  defines  the  total  additional  non-
structural mass to be distributed by an area weighted distribution to all nodes of 
a given part ID. 
•  New  keyword  option,  SET,  for  *INTIAL_STRESS_SHELL_SET  allows  a  set  of 
shells to be initialized with the state of stress. 
•  New option allows the number of cpu’s to be specified on the *KEYWORD input.   
•  Tubular drawbead box option for defining the elements that are included in the 
drawbead contact, see *DEFINE_BOX_DRAWBEAD. 
•  New  function:  *DEFINE_CURVE_DRAWBEAD,  allow  user  to  conveniently 
define drawbead by using curves (in x, y format or iges format) 
•  New function: *DEFINE_DRAWBEAD_BEAM, which allows user to convenient-
ly define drawbead by using beam part ID, and specify the drawbead force. 
•  Analytic function can be used in place of load curves with the option *DEFINE_-
CURVE_FUNCTION. 
•  Friction  can  now  be  defined  between  part  pair  using  the  *DEFINE_FRICTION 
input. 
•  New  keyword:  *DEFINE_CURVE_TRIM_3D,  to  allow  trimming  happens  based 
on blank element normal, rather than use pre-defined direction 
•  A  new  trimming  algorithm  was  added:  *DEFINE_CURVE_TRIM_NEW,  which 
allow seed node to be input and is much faster then the original algorithm. 
•  A new keyword, *DEFINE_HEX_SPOTWELD_ASSEMBLY, is available to define 
a cluster of solid elements that comprise a single spot weld. 
•  The  definition  of  a  vector,  see  *DEFINE_VECTOR,  can  be  done  by  defining 
coordinates in a local coordinate system. 
•  The  definition  of  a  failure  criteria  between  part  pairs  is  possible  with  a  table 
defined using the keyword, *DEFINE_SPOTWELD_FAILURE_RESULTANTS. 
•  A  new  keyword,  *DEFINE_CONNECTION_PROPERTIES  is  available  for 
defining failure properties of spot welds. 
•  Added  *DEFINE_SET_ADAPTIVE  to  allow  the  adaptive  level  and  element  size 
to be specified by part ID or element set ID.
INTRODUCTION 
•  Static rupture stresses for beam type spot welds can be defined in the keyword 
input, *DEFINE_SPOTWELD_RUPTURE_STRESS. 
•  Section  properties  can  be  define  in  the  *ELEMENT_BEAM  definitions  for 
resultant beam elements using the SECTION option. 
•  Physical  offsets  of  the  shell  reference  surface  can  be  specified  on  the  shell 
element cards, see the OFFSET option on *ELEMENT_SHELL. 
•  File  names  can  be  located  in  remote  directories  and  accessed  through  the  *IN-
CLUDE_PART keyword. 
•  New  features  to  *INCLUDE_STAMPED_PART:  two  different  mirror  options, 
user-defined searching radius. 
•  *INTIAL_STRESS_SECTION allows for stress initialization across a cross-section, 
which consists of solid elements.   
•  An  option,  IVATN,  is  available  for  setting  the  velocities  of  slaved  nodes  and 
parts for keyword, *INITIAL_VELOCITY_GENERATION. 
•  Twenty-two  built-in  cross-section  are  now  available  in  the  definition  of  beam 
integration rules, see *INTEGRATION_BEAM. 
•  The  possibility  of  changing  material  types  is  now  available  for  shells  using  the 
user defined integration rule, see *INTEGRATION_SHELL. 
•  The  interface  springback  file  created  by  using  the  keyword,  *INTERFACE_-
SPRINGBACK is now optionally written as a binary file. 
•  An optional input line for *KEYWORD allows the definition of a prefix for all file 
names created during a simulation.  This allows multiple jobs to be executed in 
the same directory. 
•  Body force loads can  now be applied in a  local coordinate system for *LOAD_-
BODY. 
•  A pressure loading feature allows moving pressures to be applied to a surface to 
simulate spraying a surface with stream of fluid through a nozzle.  See keyword 
*LOAD_MOVING_PRESSURE. 
•  Thermal expansion can be added to any material by the keyword, *MAT_ADD_-
THERMAL_EXPANSION. 
•  Curves  can  now  be  used  instead  of  eight  digitized  data  points  in  the  material 
model *MAT_ELASTIC_WITH_VISCOSITY_CURVE 
•  New options for spot weld failure in *MAT_SPOTWELD, which apply to beam 
and solid elements. 
•  Failure  criteria  based  on  plastic  strain  to  failure  is  added  to  material  *MAT_-
ANISOTROPIC_VISCOPLASTIC. 
•  Strain  rate  failure  criterion  is  added  to  material  *MAT_MODIFIED_PIECE-
WISE_LINEAR_PLASTICITY.
INTRODUCTION 
•  Strain rate scaling of the yield stress can now be done differently in tension and 
compression in material with separate pressure cut-offs in tension and compres-
sion in material model *MAT_PLASTICITY_TENSION_COMPRESSION. 
•  The RCDC model is now available to predict failure in material *MAT_PLASTIC-
ITY_WITH_DAMAGE. 
•  Two additional yield surfaces have been added to material *MAT_MODIFIED_-
HONEYCOMB  to  provide  more  accurate  predictions  of  the  behavior  of  honey-
comb barrier models. 
•  Unique  coordinate  systems  can  be  assigned  to  the two  nodal  points  of  material 
*MAT_1DOF_GENERALIZED_SPRING. 
•  Poisson’s  ratio  effects  are  available  in  foam  defined  by  load  curves  in  the 
material *MAT_SIMPLIFIED_RUBBER/FOAM 
•  Failure effects are available in the rubber/foam material defined by load curves 
in the *MAT_SIMPLIFIED_RUBBER/FOAM_WITH_FAILURE. 
•  The material option *MAT_ADD_EROSION now allows the maximum pressure 
at failure and the minimum principal strain at failure to be specified. 
•  Strains rather than displacements can now be used with the material model for 
discrete beams, *MAT_GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM. 
•  New  option 
for  *MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLAS-
TIC_(ECHANGE),  which  allow  two  ways  to  change  the  Young’s  modulus  dur-
ing forming simulation. 
•  New  Material  model:  *MAT_HILL_3R:  includes  the  shear  term  in  the  yield 
surface calculation by using Hill’s 1948 an-isotropic material model. 
•  New  Material  model:  *MAT_KINEMATIC_HARDENING_TRANSVERSELY_-
ANISOTROPIC: which integrates Mat #37 with Yoshida’s two-surface kinematic 
hardening model. 
•  Improved formulation for the fabric material, *MAT_FABRIC for formulations 2, 
3, and 4.  The improved formulations are types 12, 13, and 14. 
•  Constitutive models added for truss elements: 
◦  *MAT_MUSCLE 
•  For beam elements 
◦  *MAT_MOMENT_CURVATURE 
•  For shell elements 
◦  *MAT_RESULTANT_ANISOTROPIC 
◦  *MAT_RATE_SENSITIVE_COMPOSITE_FABRIC. 
◦  *MAT_SAMP-1
INTRODUCTION 
◦  *MAT_SHAPE_MEMORY is now implemented for shells. 
•  for shell and solid elements: 
◦  *MAT_BARLAT_YLD2000 for anisotropic aluminum alloys. 
◦  *MAT_SIMPLIFIED_RUBBER_WITH_DAMAGE 
◦  *MAT_VISCOELASTIC_THERMAL 
◦  *MAT_THERMO_ELASTO_VISCOPLASTIC_CREEP 
•  for the solid elements: 
◦  *MAT_ARUP_ADHESIVE 
◦  *MAT_BRAIN_LINEAR_VISCOELASTIC. 
◦  *MAT_CSCM for modeling concrete. 
◦  *MAT_PLASTICITY_COMPRESSION_TENSION_EOS for modeling ice. 
◦  *MAT_COHESIVE_ELASTIC 
◦  *MAT_COHESIVE_TH 
◦  *MAT_COHESIVE_GENERAL 
◦  *MAT_EOS_GASKET 
◦  *MAT_SIMPLIFIED_JOHNSON_COOK is now implemented for solids. 
◦  *MAT_PLASTICITY_WITH_DAMAGE is now implemented for solids. 
◦  *MAT_SPOTWELD_DAIMLERCHRYSLER 
•  User defined equations-of-state are now available. 
•  There is now an interface with the MOLDFLOW code. 
•  Damping  defined 
in  *DAMPING_PART_STIFFNESS  now  works  for  the 
Belytschko –Schwer beam element. 
•  The  option  *NODE_TRANSFORMATION  allows  a  node  set  to  be  transformed 
based on a transformation defined in *DEFINE_TRANSFORMATION. 
•  Parameters can be defined in FORTRAN like expressions using *PARAMETER_-
EXPRESSION. 
•  A part can be moved in a local coordinate system in *PART_MOVE. 
•  A  simplified  method  for  defining  composite  layups  is  available  with  *PART_-
COMPOSITE 
•  The rigid body inertia can be changed in restart via *CHANGE_RIGID_BODY_-
INERTIA. 
•  A part set can now be defined by combining other part sets in *SET_PART_ADD. 
•  Termination  of  the  calculation  is  now  possible  if  a  specified  number  of  shell 
elements  are  deleted  in  a  give  part  ID.    See  *TERMINATION_DELETED_-
SHELLS.
INTRODUCTION 
•  Added  hourglass  control  type  7  for  solid  elements  for  use  when  modeling 
hyperelastic materials. 
•  Shell formulations 4, 11, 16, and 17 can now model rubber materials. 
•  Added  a  new  seatbelt  pretensioner  type  7  in  which  the  pretensioner  and 
retractor forces are calculated independently and added. 
•  A  new  composite  tetrahedron  element  made  up  from  12  tetrahedron  is  now 
available as solid element type 17. 
•  Shell thickness offsets for *SECTION_SHELL now works for most shell elements, 
not just the Hughes-Liu shell. 
•  The  Hughes-Liu  beam  has  been  extended  to  include  warpage  for  open  cross-
sections. 
•  A resultant beam formulation with warpage is available as beam type 12. 
•  Two nonlinear shell elements are available  with 8 degrees-of-freedom per node 
to include thickness stretch. 
•  Tetrahedron  type  13,  which  uses  nodal  pressures,  is  now  implemented  for 
implicit applications. 
•  Cohesive solid elements are now available for treating failure. 
•  Seatbelt shell elements are available for use with the all seatbelt capabilities. 
•  Superelements  can  now  share  degrees-of-freedom  and  are  implemented  for 
implicit applications under MPI. 
•  A user defined element interface is available for solid and shell elements. 
•  Thermal shells are available for treating heat flow through shell elements. 
•  EFG shell formulations 41 and 42 are implemented for explicit analysis. 
•  EFGPACK  is  implemented  in  addition  to  BCSLIB-EXT  solver  on  the  keyword 
*CONTROL_EFG. 
•  EFG MPP version is available for explicit analysis. 
•  EFG fast transformation method is implemented in the EFG solid formulation.   
•  EFG Semi-Lagrangian kernel and Eulerian kernel options are added for the foam 
materials.   
•  EFG 3D adaptivity is implemented for the metal materials. 
•  EFG E.O.S.  and *MAT_ELASTIC_FLUID materials are included in the 4-noded 
background element formulation.   
•  Airbag  simulations  by  using  ALE  method  can  be  switched  to  control  volume 
method by *ALE_CV_SWITCH.   
•  *MAT_ALE_VISCOUS now supports Non-Newtonian viscosity by power law or 
load curve.
INTRODUCTION 
•  *DATABASE_BINARY_FSIFOR  outputs  fluid-structure 
interaction  data  to 
binary file. 
•  *DATABASE_FSI_SENSOR outputs ALE element pressure to ASCII file dbsor. 
•  *MAT_GAS_MIXTURE supports nonlinear heat capacities. 
•  *INITIAL_VOLUME_FRACTION_GEOMETRY  uses  an  enhanced  algorithm  to 
handle both concave and convex geometries and substantially reduce run time. 
•  A new keyword *DELETE_FSI allows the deletion of coupling definitions. 
•  Convection  heat  transfer  activates  by  *LOAD_ALE_CONVECTION  in  ALE  FSI 
analysis. 
•  *ALE_FSI_SWITCH_MMG  is  implemented  to  switch  between  ALE  multi-
material groups to treat immersed FSI problems. 
•  Type  9  option  is  added  in  *ALE_REFERENCE_SYSTEM_GROUP  to  deal 
complex  ALE  mesh  motions  including  translation,  rotation,  expansion  and 
contraction, etc. 
◦  New options in *CONSTRAINED_LAGRANGE_IN_SOLID 
◦  Shell thickness option for coupling type 4. 
◦  Bulk modulus based coupling stiffness. 
◦  Shell erosion treatment. 
◦  Enable/disable interface force file.   
•  New coupling method for fluid flowing through porous media are implemented 
as type 11 (shell) and type 12 (solid) in *CONSTRAINED_LAGRANGE_IN_SOL-
ID. 
•  *ALE_MODIFIED_STRAIN allows multiple strain fields in certain ALE elements 
to solve sticking behavior in FSI.  (MPP underdevelopment) 
•  *ALE_FSI_PROJECTION is added as a new constraint coupling method to solve 
small pressure variation problem.  (MPP underdevelopment) 
•  *BOUNDARY_PRESCRIBED_ORIENTATION_RIGID  is  added  as  a  means  to 
prescribe  as  a  function  of  time  the  general  orientation  of  a  rigid  body  using  a 
variety of methods.  This feature is available in release R3 and higher of Version 
971. 
•  *BOUNDARY_PRESCRIBED_ACCELEROMETER_RIGID is added as a means to 
prescribe the motion of a rigid body based un experimental data gathered from 
accelerometers  affixed  to  the  rigid  body.    This  feature  is  available  in  release  R3 
and higher of Version 971.
INTRODUCTION 
Capabilities added during 2008-2011 for Version 971R6 of LS-DYNA: 
During the last four years the implicit capabilities are now scalable to a large number of 
cores;  therefore,  LS-DYNA  has  achieved  a  major  goal  over  15  years  of  embedding  a 
scalable  implicit  solver.    Also,  in  addition  to  the  progress  made  for  implicit  solutions 
many other new and useful capabilities are now available. 
•  The  keyword  *ALE_AMBIENT_HYDROSTATIC 
initializes  the  hydrostatic 
pressure field in the ambient ALE domain due to an acceleration like gravity. 
•  The  keyword  *ALE_FAIL_SWITCH_MMG  allows  switching  an  ALE  multi-
material-group ID (AMMGID) if the material failure criteria occurs.   
•  The  keyword  *ALE_FRAGMENTATION  allow  switching  from  the  ALE  multi-
material-group ID, AMMGID, (FR_MMG) of this failed material to another AM-
MGID (TO_MMG).  This feature may typically be used in simulating fragmenta-
tion of materials. 
•  The keyword *ALE_REFINE refines ALE hexahedral solid elements automatical-
ly.   
•  The  keyword  *BOUNDARY_ALE_MAPPING  maps  ALE  data  histories  from  a 
previous  run  to  a  region  of  elements.    Data  are  read  from  or  written  to  a  map-
ping  file  with  a  file  name  given  by  the  prompt  “map=”  on  the  command  line 
starting the execution. 
•  The  keyword  *BOUNDARY_PORE_FLUID  is  used  to  define  parts  that  contain 
pore fluid where defaults are given on *CONTROL_PORE_FLUID input. 
•  With  the  keyword,  *BOUNDARY_PRESCRIBED_FINAL_GEOMETRY,  the  final 
displaced  geometry  for  a  subset  of  nodal  points  is  defined.    The  nodes  of  this 
subset are displaced from their initial positions specified in the *NODE input to 
the final geometry along a straight line trajectory.  A load curve defines a scale 
factor as a function of time that is bounded between zero and unity correspond-
ing  to  the  initial  and  final  geometry,  respectively.    A  unique  load  curve  can  be 
specified for each node, or a default load curve can apply to all nodes.   
•  The  keyword,  *BOUNDARY_PWP,  defines  pressure  boundary  conditions  for 
pore water at the surface of the software.   
•  The  keyword,  *CONSTRAINED_JOINT_COOR,  defines  a  joint  between  two 
rigid bodies.  The connection coordinates are given instead of the nodal point IDs 
used in *CONSTRAINED_JOINT. 
•  The keyword, *CONSTRAINED_SPR2, defines a self-piercing rivet with failure.  
This model for a self-piercing rivet (SPR2) includes a plastic-like damage model 
that  reduces  the  force  and  moment  resultants  to  zero  as  the  rivet  fails.    The 
domain of influence  is specified by a diameter, which  should  be approximately 
equal to the rivet’s diameter.  The location of the rivet is defined by a single node 
at the center of two riveted sheets.
INTRODUCTION 
•  Through  the  keyword,  *CONTROL_BULK_VISCOSITY,  bulk  viscosity 
is 
optional for the Hughes-Liu beam and beam type 11 with warpage.  This option 
often provides better stability, especially in elastic response problems. 
•  The display of nodal rigid bodies is activated by the parameter, PLOTEL, on the 
*CONTROL_RIGID keyword.   
•  The mortar contact, invoked by appending the suffix MORTAR to either FORM-
ING_SURFACE_TO_SURFACE,  AUTOMATIC_SURFACE_TO_SURFACE  or 
AUTOMATIC_SINGLE_SURFACE,  is  a  segment  to  segment  penalty  based 
contact.  For two segments on each side of the contact interface that are overlap-
ping and penetrating, a consistent nodal force assembly taking into account the 
individual  shape  functions  of  the  segments  is  performed.    In  this  respect  the 
results  with  this  contact  may  be  more  accurate,  especially  when  considering 
contact  with  elements  of  higher  order.    By  appending  the  suffix  TIED  to  the 
CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_MORTAR  keyword  or 
the  suffix  MORTAR  to  the  CONTACT_AUTOMATIC_SURFACE_TO_SUR-
FACE_TIEBREAK  keyword,  this  is  treated  as  a  tied  contact  interface  with  tie-
break  failure  in  the  latter  case.    Only  OPTION = 9  is  supported  for  the  mortar 
tiebreak contact.  The mortar contact is intended for implicit analysis in particu-
lar but is nevertheless supported for explicit analysis as well. 
•  In  the  database,  ELOUT,  the  number  of  history  variables  can  be  specified  for 
output each integration point in the solid, shell, thick shell, and beam elements.  
The  number  of  variables  is  given  on  the  *DATABASE_ELOUT  keyword  defini-
tion. 
•  A  new  option  is  available  in  *DATABASE_EXTENT_BINARY.    Until  now  only 
one  set  of  integration  points  were  output  through  the  shell  thickness.      The 
lamina  stresses  and  history  variables  were  averaged  for  fully  integrated  shell 
elements,  which  results  in  less  disk  space  for  the  D3PLOT  family  of  files,  but 
makes it difficult to verify the accuracy of the stress calculation after averaging.  
An  option  is  now  available  to  output  all  integration  point  stresses  in  fully  inte-
grated shell elements: 4 x # of through thickness integration points in shell types 
6, 7, 16, 18-21, and 3 x # of through thickness integration points in triangular shell 
types 3, and 17.   
•  The  keyword  *DATABASE_PROFILE  allows  plotting  the  distribution  or  profile 
of data along x, y, or z-direction. 
•  The  purpose  of  the  keyword,  *DEFINE_ADAPTIVE_SOLID_TO_SPH,  is  to 
adaptively transform a Lagrangian solid Part or Part Set to SPH particles when 
the  Lagrange  solid  elements  comprising  those  parts  fail.    One  or  more  SPH 
particles (elements) will be generated for each failed element to.  The SPH parti-
cles  replacing  the  failed  element  inherit  all  of  the  properties  of  failed  solid  ele-
ment, e.g.  mass, kinematic variables, and constitutive properties.
INTRODUCTION 
•  With  the  keywords  beginning  with,  *DEFINE_BOX,  a  LOCAL  option  is  now 
available.  With this option the diagonal corner coordinates are given in a local 
coordinate system defined by an origin and vector pair. 
•  The  keyword,  *DEFINE_CURVE_DUPLICATE,  defines  a  curve  by  optionally 
scaling and offsetting the abscissa and ordinates of another curve defined by the 
*DEFINE_CURVE keyword. 
•  The  keyword,  *DEFINE_ELEMENT_DEATH,  is  available  to  delete  a  single 
element or an element set at a specified time during the calculation.   
•  The purpose of the keyword, *DEFINE_FRICTION_ORIENTATION, is to allow 
for the definition of different coefficients of friction (COF) in specific directions, 
specified  using  a  vector  and  angles  in  degrees.    In  addition,  COF  can  be  scaled 
according to the amount of pressure generated in the contact interface.   
•  With  the  new  keyword,  *DEFINE_FUNCTION,  an  arithmetic  expression 
involving a combination of independent variables and other functions, i.e., 
f(a,b,c) = a*2 + b*c + sqrt(a*c) 
is  defined  where  a,  b,  and  c  are  the  independent  variables.    This  option  is  im-
plemented for a subset of keywords. 
◦  *ELEMENT_SEATBELT_SLIPRING 
◦  *LOAD_BEAM 
◦  *LOAD_MOTION_NODE 
◦  *LOAD_MOVING_PRESSURE 
◦  *LOAD_NODE 
◦  *LOAD_SEGMENT 
◦  *LOAD_SEGMENT_NONUNIFORM 
◦  *LOAD_SETMENT_SET_NONUNIFORM 
◦  *BOUNDARY_PRESCRIBED_MOTION  
•  If a curve ID is not found, then the function ID’s are checked. 
•  The  keyword,  *DEFINE_SPH_TO_SPH_COUPLING,    defines  a  penalty  based 
contact  to be used for the node to node contacts between SPH parts. 
•  The keyword, *DEFINE_TABLE_2D, permits the same curve ID to be referenced 
by multiple tables, and the curves may be defined anywhere in the input. 
•  The  keyword,  *DEFINE_TABLE_3D,  provides  a  way  of  defining  a  three-
dimensional table.  A 2D table ID is specified for each abscissa value defined for 
the 3D table. 
•  The keyword, *ELEMENT_BEAM_PULLEY, allows the definition of a pulley for 
truss  beam  elements    .    Currently,  the 
beam  pulley  is  implemented  for    *MAT_001  and  *MAT_156.      Pulleys  allow 
continuous sliding of a string of truss beam element through a sharp change of 
angle.
INTRODUCTION 
•  The  purpose  of  the  keyword,  *ELEMENT_MASS_MATRIX,  is  to  define  a  6x6 
symmetric  nodal  mass  matrix  assigned  to  a  nodal  point  or  each  node  within  a 
node set. 
•  The  keyword,  *ELEMENT_DISCRETE_SPHERE,  allows  the  definition  of  a 
discrete  spherical  element  for  discrete  element  calculations.    Each  particle  con-
sists of a single node with its mass, mass moment of inertia, and radius.  Initial 
coordinates and velocities are specified via the nodal data.   
•  The 
two  keywords,  *ELEMENT_SHELL_COMPOSITE  and  *ELEMENT_-
TSHELL_COMPOSITE, are used to define elements for a general composite shell 
part where the shells within the part can have an arbitrary number of layers.  The 
material ID, thickness, and material angle are specified for the thickness integra-
tion points for each shell in the part 
•  The  keyword,  *EOS_USER_DEFINED,  allows  a  user  to  supply  their  own 
equation-of-state subroutine. 
•  The  new  keyword  *FREQUENCY_DOMAIN  provides  a  way  of  defining  and 
solving  frequency  domain  vibration  and  acoustic  problems.    The  related  key-
word cards given in alphabetical order are: 
◦  *FREQUENCY_DOMAIN_ACOUSTIC_BEM_{OPTION} 
◦  *FREQUENCY_DOMAIN_ACOUSTIC_FEM 
◦  *FREQUENCY_DOMAIN_FRF 
◦  *FREQUENCY_DOMAIN_RANDOM_VIBRATION 
◦  *FREQUENCY_DOMAIN_RESPONSE_SPECTRUM 
◦  *FREQUENCY_DOMAIN_SSD 
•  The  keyword,  *INITIAL_AIRBAG_PARTICLE,  initializes  pressure  in  a  closed 
airbag volume, door cavities for pressure sensing studies, and tires. 
•  The  keyword  *INITIAL_ALE_HYDROSTATIC 
initializes 
the  hydrostatic 
pressure field in an ALE domain due to an acceleration like gravity. 
•  The  keyword  *INITIAL_ALE_MAPPING  maps  ALE  data  histories  from  a 
previous run.  Data are read from a mapping file with a file name given by the 
prompt “map=” on the command line starting the execution. 
•  The  keyword,  *INITIAL_AXIAL_FORCE_BEAM,  provides  a  simplified  method 
to model initial tensile forces in bolts. 
•  The keyword, *INITIAL_FIELD_SOLID, is a simplified version of the *INITIAL_-
STRESS_SOLID  keyword  which  can  be  used  with  hyperelastic  materials.    This 
keyword  is  used  for  history  variable  input.    Data  is  usually  in  the  form  of  the 
eigenvalues  of  diffusion  tensor  data.    These  are  expressed  in  the  global  coordi-
nate system.   
•  The  equation-of-state,  *EOS_MIE_GRUNEISEN,  type  16,  is  a  Mie-Gruneisen 
form with a p-α compaction model.
INTRODUCTION 
•  The keyword, *LOAD_BLAST_ENHANCED, defines an air blast function for the 
application  of  pressure  loads  due  the  explosion  of  conventional  charge.    While 
similar to *LOAD_BLAST this feature includes enhancements for treating reflect-
ed waves, moving warheads and multiple blast sources.  The loads are applied to 
facets  defined  with  the  keyword  *LOAD_BLAST_SEGMENT.    A  database  con-
taining blast pressure history is also available . 
•  The  keyword,  *LOAD_ERODING_PART_SET,  creates  pressure  loads  on  the 
exposed  surface  composed  of  solid  elements  that  erode,  i.e.,  pressure  loads  are 
added to newly exposed surface segments as solid elements erode. 
•  The  keyword,  *LOAD_SEGMENT_SET_ANGLE,  applies  traction  loads  over  a 
segment set that is dependent on the orientation of a vector.  An example appli-
cation is applying a pressure to a cylinder as a function of the crank angle in an 
automobile engine 
•  The  keyword,  *LOAD_STEADY_STATE_ROLLING,  is  a  generalization  of 
*LOAD_BODY, allowing the user to apply body loads to part sets due to transla-
tional  and  rotational  accelerations  in  a  manner  that  is  more  general  than  the 
*LOAD_BODY  capability.    The  *LOAD_STEADY_STATE_ROLLING  keyword 
may be invoked an arbitrary number of times in the problem as long as no part 
has  the  option  applied  more  than  once  and  they  can  be  applied  to  arbitrary 
meshes.  This option is frequently used to initialize stresses in tire. 
•  The  keywords  INTERFACE_SSI,  INTERFACE_SSI_AUX,  INTERFACE_SSI_-
AUX_EMBEDDED  and  INTERFACE_SSI_STATIC  are  used  to  define  the  soil-
structure  interface  appropriately  in  various  stages  of  soil-structure  interaction 
analysis under earthquake ground motion.   
•  The  keyword,  *LOAD_SEISMIC_SSI,  is  used  to  apply  earthquake  loads  due  to 
free-field  earthquake  ground  motion  at  certain  locations  —  defined  by  either 
nodes  or  coordinates  —  on  a  soil-structure  interface.    This  loading  is  used  in 
earthquake soil-structure interaction analysis.  The specified motions are used to 
compute a set of effective forces in the soil elements adjacent to the soil-structure 
interface, according to the effective seismic input–domain reduction method. 
•  The keyword *DEFINE_GROUND_MOTION is used to specify a ground motion 
to be used in conjunction with *LOAD_SEISMIC_SSI. 
•  Material  types  *MAT_005  and  *MAT_057  now  accept  table  input  to  allow  the 
stress quantity versus the strain measure to be  defined as a function of tempera-
ture. 
•  The  material  option  *MAT_ADD_EROSION,  can  now  be  applied  to  all 
nonlinear  shell,  thick  shell,  fully  integrated  solids,  and  2D  solids.    New  failure 
criteria are available. 
•  The  GISSMO  damage  model,  now  available  as  an  option  in  *MAT_ADD_ERO-
SION, is a phenomenological formulation that allows for an incremental descrip-
INTRODUCTION 
tion of damage accumulation, including softening and failure.  It is intended to 
provide a maximum in variability for the description of damage for a variety of 
metallic  materials  (e.g.    *MAT_024,  *MAT_036, …).    The  input  of  parameters  is 
based on tabulated data, allowing the user to directly convert test data to numer-
ical input. 
•  The  keyword,  *MAT_RIGID_DISCRETE  or  MAT_220,  eliminates  the  need  to 
define  a  unique  rigid  body  for  each  particle  when  modeling  a  large  number  of 
rigid particles.  This gives a large reduction in memory and wall clock time over 
separate rigid bodies.  A single rigid material is defined which contains multiple 
disjoint pieces.  Input is simple and unchanged, since all disjoint rigid pieces are 
identified automatically during initialization. 
•  The  keyword,  *NODE_MERGE,  causes  nodes  with  identical  coordinates  to  be 
replaced  during  the  input  phase  by  the  node  encountered  that  has  the  smallest 
ID.    
•  The keyword, *PART_ANNEAL, is used to initialize the stress states at integra-
tion points within a specified part to zero at a given time during the calculation.  
This  option  is  valid  for  parts  that  use  constitutive  models  where  the  stress  is 
incrementally  updated.    This  option  also  applies  to  the  Hughes-Liu  beam  ele-
ments, the integrated shell elements, thick shell elements, and solid elements. 
•  The  keyword,  *PART_DUPLICATE,  provides  a  method  of  duplicating  parts  or 
part sets without the need to use the *INCLUDE_TRANSFORM option.   
•  To automatically generate elements to visualize rigid walls the DISPLAY option 
is now available for *RIGIDWALL_PLANAR and *RIGIDWALL_GEOMETRIC. 
•  A  one  point  integrated  pentahedron  solid  element  with  hourglass  control  is 
implemented  as  element  type  115  and  can  be  referenced  in  *SECTION_SOLID.  
Also, the 2 point pentahedron solid, type 15, no longer has a singular mode. 
•  The  keyword  *SECTION_ALE1D  defines  section  properties  for  1D  ALE 
elements. 
•  The  keyword  *SECTION_ALE2D  defines  section  properties  for  2D  ALE 
elements. 
•  The keywords *SET_BEAM_INTERSECT, *SET_SHELL_INTERSECT, *SET_SOL-
ID_INTERSECT, *SET_NODE_INTERSECT, and *SET_SEGMENT_INTER-SECT, 
allows the definition of a set as the intersection, ∩, of a series of sets.  The new 
set, SID, contains all common members.   
•  The  keyword,  *SET_SEGMENT_ADD,  is  now  available  for  defining  a  new 
segment set by combining other segment sets.   
•  The  two  keywords,  *DEFINE_ELEMENT_GENERALIZED_SHELL  and  *DE-
FINE_ 
ELEMENT_GENERALIZED_SOLID,  are  used  to  define  general  shell  and  solid 
element  formulations  to  allow  the  rapid  prototyping  of  new  element  formula-
INTRODUCTION 
tions.  They are used in combination with the new keywords *ELEMENT_GEN-
ERLIZED_SHELL and *ELEMENT_GENERALIZED_SOLID. 
•  The two keywords, *ELEMENT_INTERPOLATION_SHELL and *ELEMENT_ 
INTERPOLATION_SOLID,  are  used  to  interpolate  stresses  and  other  solution 
variables from the generalized shell and solid element formulations for visualiza-
tion.  They are used together with the new keyword *CONSTRAINED_NODE_-
INTERPOLATION. 
•  The  keyword,  *ELEMENT_SHELL_NURBS_PATCH,  is  used  to  define  3D  shell 
elements  based  on  NURBS  (Non-Uniform  Ration  B-Spline)  basis  functions.  
Currently  four  different  element  formulations,  with  and  without  rotational 
degrees of freedom are available. 
•  The  keyword  LOAD_SPCFORC  is  used  to  apply  equivalent  SPC  loads,  read  in 
from  the  d3dump  file  during  a  full-deck  restart,  in  place  of  the  original  con-
straints in order to facilitate the classical non-reflecting boundary on an outside 
surface. 
Capabilities added in 2012 to create Version 97R6.1, of LS-DYNA: 
•  A  new  keyword 
*MAT_THERMAL_DISCRETE_BEAM  defines 
thermal 
properties for ELFORM 6 beam elements. 
•  An  option  *CONTROL_THERMAL_SOLVER,  invoked  by  TSF < 0,  gives  the 
thermal  speedup  factor  via  a  curve.    This  feature  is  useful  when  artificially 
scaling velocity in metal forming.   
•  A  nonlinear  form  of  Darcy's  law  in  *MAT_ADD_PORE_AIR  allows  curves  to 
define  the  relationship  between  pore  air  flow  velocity  and  pore  air  pressure 
gradient. 
•  An  extention  to  the  PART  option  in  *SET_SEGMENT_GENERAL  allows 
reference  to  a  beam  part.    This  allows  for  creation  of  2D  segments  for  traction 
application. 
•  Options  “SET_SHELL”,  “SET_SOLID”,  “SET_BEAM”,  “SET_TSHELL”,  “SET_-
SPRING”  are  added  to  *SET_NODE_GENERAL  so  users  can  define  a  node  set 
using existing element sets. 
•  Options  “SET_SHELL”,  “SET_SOLID”,  “SET_SLDIO”,  “SET_TSHELL”,  “SET_-
TSHIO”  are  added  to  *SET_SEGMENT_GENERAL  so  users  can  use  existing 
element sets to define a segment set. 
•  *BOUNDARY_PRESCRIBED_MOTION_SET_BOX  prescribes  motion  to  nodes 
that fall inside a defined box. 
•  IPNINT > 1  in  *CONTROL_OUTPUT  causes  d3hsp  to  list  the  IPNINT  smallest 
element timesteps in ascending order. 
•  Section and material titles are echoed to d3hsp.
INTRODUCTION 
•  A new parameter MOARFL in *DEFINE_CONNECTION_PROPERTIES permits 
reduction in modeled area due to shear. 
•  A  new  option  HALF_SPACE  in  *FREQUENCY_DOMAIN_ACOUSTIC_BEM 
enables  treatment  of  a  half-space  in  boundary  element  method,  frequency  do-
main acoustic analysis. 
•  A shell script “kill_by_pid” is created during MPP startup.  When executed, this 
script  will  run  “kill  -9”  on  every  LS-DYNA  process  started  as  part  of  the  MPP 
job.    This  is  for  use  at  the  end  of  submission  scripts,  as  a  “fail  safe”  cleanup  in 
case the job aborts. 
•  A  new  parameter  IAVIS  in  *CONTROL_SPH  selects  the  artificial  viscosity 
formulation for the SPH particles.  If set to 0, the Monaghan type artificial viscos-
ity  formulation  is  used.    If  set  to  1,  the  standard  artificial  viscosity  formulation 
for solid elements is used which may provide a better energy balance but is less 
stable in specific applications such as high velocity impact. 
•  Contact  friction  may  be  included  in  *CONTACT_2D_NODE_TO_SOLID  for 
SPH. 
•  A  new  keyword  *ALE_COUPLING_NODAL_CONSTRAINT  provides  a 
coupling mechanism between ALE solids and non-ALE nodes.  The nodes can be 
from  virtually  any  non-ALE  element  type  including  DISCRETE_SPHERE,  EFG, 
and SPH, as well as the standard Lagrangian element types.  In many cases, this 
coupling  type  may  be  a  better  alternative  to  *CONSTRAINED_LAGRANGE_-
IN_SOLID. 
•  The  keyword  *ALE_ESSENTIAL_BOUNDARY  assigns  essential  boundary 
conditions to nodes of the ALE boundary surface.  The command can be repeat-
ed multiple times and is recommended over use of EBC in *CONTROL_ALE.. 
•  The keyword *DELETE_ALECPL in a small restart deck deletes coupling defined 
with  *ALE_COUPLING_NODAL_CONSTRAINT.    The  command  can  also  be 
used to reinstate the coupling in a later restart. 
•  *DEFINE_VECTOR_NODES defines a vector with two node points. 
•  *CONTACT_AUTOMATIC_SINGLE_SURFACE_TIED allows for the calculation 
of  eigenvalues  and  eigenvectors  for  models  that  include  *CONTACT_AUTO-
MATIC_SINGLE_SURFACE. 
•  A new parameter RBSMS in *CONTROL_RIGID affects rigid body treatment in 
Selective Mass Scaling (*CONTROL_TIMESTEP).  When rigid bodies are in any 
manner connected to deformable elements, RBSMS = 0 (default) results in spuri-
ous inertia due to improper treatment of the nodes at the interface.  RBSMS = 1 
alleviates this effect but an additional cost is incurred. 
•  A  new  parameter  T10JTOL  in  *CONTROL_SOLID  sets  a  tolerance for  issuing  a 
warning  when  J_min/J_max  goes  below  this  tolerance  value  (i.e.,  quotient 
between  minimum  and  maximum  Jacobian  value  in  the  integration  points)  for
INTRODUCTION 
tetrahedron  type  16.    This  quotient  serves  as  an  indicator  of  poor  tetrahedral 
element meshes in implicit that might cause convergence problems. 
•  A new option MISMATCH for *BOUNDARY_ACOUSTIC_COUPLING handles 
coupling of structural element faces and acoustic volume elements (ELFORMs 8 
and 14) in the case where the coupling surfaces do not have coincident nodes. 
•  A  porosity  leakage  formulation  in  *MAT_FABRIC  (*MAT_034,  FLC < 0)  is  now 
available for  particle gas airbags (*AIRBAG_PARTICLE). 
•  *BOUNDARY_PRESCRIBED_ACCELEROMETER  is  disabled  during  dynamic 
relaxation. 
•  A  new  parameter  CVRPER  in  *BOUNDARY_PAP  defines  porosity  of  a  cover 
material encasing a solid part. 
•  A  parameter  TIEDID  in  *CONTACT_TIED_SURFACE_TO_SURFACE  offers  an 
optional incremental normal update in SMP to eliminate spurious contact forces 
that may appear in some applications. 
•  A new option SPOTSTP = 3 in *CONTROL_CONTACT retains spot welds even 
when the spot welds are not found by *CONTACT_SPOTWELD. 
•  The SMP consistency option (ncpu < 0) now pertains to the ORTHO_FRICTION 
contact option. 
•  Forces  from  *CONTACT_GUIDED_CABLE  are  now  written  to  ncforc  (both 
ASCII and binout). 
•  Discrete beam materials 70, 71, 74, 94, 121 calculate axial force based on change 
in  length.    Output  the  change  in  length  instead  of  zero  axial  relative  displace-
ment to ASCII file disbout (*DATABASE_DISBOUT). 
•  *DATABASE_RCFORC_MOMENT is now supported in implicit. 
•  After  the  first  implicit  step,  the  output of  projected  cpu  and  wall  clock  times  is 
written and the termination time is echoed. 
•  *DATABASE_MASSOUT  is  upgraded  to  include  a  summary  table  and  to 
optionally add mass for nodes belonging to rigid bodies. 
•  Generate and store resultant forces for the LaGrange Multiplier joint formulation 
so as to give correct output to  jntforc (*DATABASE_JNTFORC). 
•  Control the number of messages for deleted and failed elements using parameter 
MSGMAX in *CONTROL_OUTPUT. 
•  Nodal  and  resultant  force  output  is  written  to  nodfor  for  nodes  defined  in 
*FREQUENCY_DOMAIN_SSD 
in 
*DATABASE_NODAL_FORCE_GROUP 
analysis (SMP only). 
•  Ncforc data is now written for guided cables (*CONTACT_GUIDED_CABLE) in 
MPP.
INTRODUCTION 
•  Jobid handling is improved in l2a utility so that binout files from multiple jobs, 
with or without a jobid-prefix, can be converted with the single command “l2a -j 
*binout*”.  The output contains the correct prefix according to the jobid. 
•  ALE_MULTI-MATERIAL_GROUP  (AMMG)  info  is  written  to  matsum  (both 
ASCII and binout). 
•  Shell  formulation  14  is  switched  to  15  (*SECTION_SHELL)  in  models  that 
include axisymmetric SPH. 
•  *ELEMENT_BEAM_PULLEY  is  permitted  with  *MAT_CABLE_DISCRETE_-
BEAM. 
•  A warning during initialization is written if a user creates DKT triangles, either 
by  ELFORM = 17  on  *SECTION_SHELL  or  ESORT = 2  on  *CONTROL_SHELL, 
that are thicker than the maximum edge length.   
•  Account  is  taken  of  degenerate  acoustic  elements  with  ELFORM  8.    Tria  and 
quad  faces  at  acoustic-structure  boundary  are  handled  appropriately  according 
to shape. 
•  The  compression  elimination  option  for  2D  seatbelts,  CSE = 2  in  *MAT_SEAT-
BELT is improved. 
•  Detailed  material  failure  (*MAT_ADD_EROSION)  messages  in  messag  and 
d3hsp  are  suppressed  when  number  of  messages > MSGMAX  (*CONTROL_-
OUTPUT). 
•  Implement  SMP  consistency 
(*MAT_186) solids and shells. 
(ncpu < 0) 
in  *MAT_COHESIVE_GENERAL 
•  Viscoelastic  model  in  *MAT_077_O  now  allows  up  to  twelve  terms  in  Prony 
series instead of standard six. 
•  Large curve ID's for friction table (*CONTACT_… with FS = 2) are enabled. 
•  Efficiency of GISSMO damage in *MAT_ADD_EROSION is improved.   
•  *MAT_ADD_PERMEABILITY_ORTHOTROPIC 
is  now  available 
for  pore 
pressure analysis (*…_PORE_FLUID). 
•  For *MAT_224 solids and shells, material damage serves as the failure variable in 
*CONSTRAINED_TIED_NODES_FAILURE. 
•  The behavior of *MAT_ACOUSTIC is modified when used in combination with 
dynamic relaxation (DR).  Acoustic domain now remains unperturbed in the DR 
phase but hydrostatic pressure from the acoustic domain is applied to the struc-
ture during DR. 
•  Option for 3D to 2D mapping is added in *INITIAL_ALE_MAPPING. 
•  *CONTACT_ERODING_NODES_TO_SURFACE contact may be used with SPH 
particles.
INTRODUCTION 
•  Total  Lagrangian  SPH  formulation  7  (*CONTROL_SPH)  is  now  available  in 
MPP. 
•  The  output  formats  for  linear  equation  solver  statistics  now  accommodate  very 
large numbers as seen in large models. 
•  *CONTROL_OUTPUT keyword parameter NPOPT is now applicable to thermal 
data.    If  NPOPT = 1,  then  printing  of  the  following  input  data  to d3hsp  is  sup-
pressed: 
◦  *INITIAL_TEMPERATURE 
◦  *BOUNDARY_TEMPERATURE 
◦  *BOUNDARY_FLUX 
◦  *BOUNDARY_CONVECTION 
◦  *BOUNDARY_RADIATION 
◦  *BOUNDARY_ENCLOSURE_RADIATION 
•  Beam energy balance information is written to TPRINT file. 
•  MPP performance for LS-DYNA/Madymo coupling is improved. 
•  Shell adaptivity (*CONTROL_ADAPTIVE) is improved to reduce the number of 
elements along curved surfaces in forming simulations. 
•  One-step  unfolding 
(*CONTROL_FORMING_ONESTEP) 
is 
improved 
to 
accommodate blanks with small initial holes. 
•  Efficiency of FORM 3 isogeometric shells is improved. 
•  The processing of *SET_xxx_GENERAL is faster. 
•  *KEYWORD_JOBID now works even when using the *CASE command. 
•  Parts may be repositioned in a small restart by including *DEFINE_TRANSFOR-
MATION and *NODE_TRANSFORM in the small restart deck to move nodes of 
a specified node set prior to continuing the simulation. 
Capabilities added during 2012/2013 to create LS-DYNA R7.0: 
•  Three solvers, EM, CESE, and ICFD, and a volume mesher to support the latter 
two solvers, are new in Version 7.  Brief descriptions of those solvers are given 
below.    Keyword  commands  for  the  new  solvers  are  in  Volume  III  of  the  LS-
DYNA Keyword User’s Manual.  These new solvers are only included in double 
precision executables. 
•  Keyword family: *EM_, the keywords starting with *EM refer to and control the 
Electromagnetic solver problem set up: 
◦  EM Solver Characteristics: 
  Implicit
INTRODUCTION 
  Double precision 
  Dynamic memory handling 
  SMP and MPP 
  2D axisymmetric solver / 3D solver 
  Automatic coupling with structural and thermal LS-DYNA solvers 
  FEM for conducting pieces only, no air mesh needed (FEM-BEM sys-
tem) 
  Solid elements for conductors, shells can be insulators 
◦  EM Solver Main Features: 
  Eddy Current (a.k.a Induction-Diffusion) solver 
  Induced heating solver 
  Resistive heating solver 
  Imposed tension or current circuits 
  Exterior field 
  Magnetic materials (beta version) 
  Electromagnetic contact 
  EM Equation of states (Conductivity as a function of temperature) 
◦  EM Solver Applications (Non-exhaustive) : 
  Electromagnetic forming 
  Electromagnetic welding 
  Electromagnetic bending 
  Inductive heating 
  Resistive heating 
  Rail-gun 
  Ring expansions 
•  Keyword family: *CESE_, the keywords starting with *CESE refer to and control 
the Compressible CFD solver problem set up: 
◦  CESE Solver Characteristics: 
  Explicit 
  Double precision 
  Dynamic memory handling 
  SMP and MPP 
  3D solver / special case 2D solver and 2D axisymmetric solver 
  Automatic coupling with structural and thermal LS-DYNA solvers 
  Eulerian  fixed  mesh  or  moving  mesh  (Either  type  input  with  *ELE-
MENT_SOLID cards or using *MESH cards) 
◦  CESE Solver Main Features:
INTRODUCTION 
  The  CESE  (Conservation  Element  /  Solution  Element)  method  en-
forces conservation in space-time  
  Highly accurate shock wave capturing 
  Cavitation model 
  Embedded  (immersed)  boundary  approach  or  moving  (fitting)  ap-
proach for FSI problems 
  Coupled stochastic fuel spray solver  
  Coupling with chemistry  solver 
◦  CESE Solver Applications (Non-exhaustive) : 
  Shock wave capturing 
  Shock/acoustic wave interaction 
  Cavitating flows 
  Conjugate heat transfer problems 
  Many  different  kinds  of  stochastic  particle  flows,  e.g,  dust,  water, 
fuel. 
  Chemically  reacting  flows,  e.g,  detonating  flow,  supersonic  combus-
tion. 
•  Keyword family: *ICFD_, the keywords starting with *ICFD refer to and control 
the incompressible CFD solver problem set up: 
◦  ICFD Solver Characteristics: 
  Implicit 
  Double precision 
  Dynamic memory handling 
  SMP and MPP 
  2D solver / 3D solver 
  Makes use of an automatic volume mesh generator for fluid domain 
 
  Coupling with structural and thermal LS-DYNA solvers   
◦  ICFD Solver Main Features: 
  Incompressible fluid solver 
  Thermal solver for fluids 
  Free Surface flows 
  Two-phase flows 
  Turbulence models 
  Transient or steady-state problems 
  Non-Newtonian fluids 
  Boussinesq model for convection 
  Loose or strong coupling for FSI (Fluid-structure interaction) 
  Exact boundary condition imposition for FSI problems
INTRODUCTION 
◦  ICFD Solver Applications (Non-exhaustive) : 
  External aerodynamics for incompressible flows 
  Internal aerodynamics for incompressible flows 
  Sloshing, Slamming and Wave impacts 
  FSI problems 
  Conjugate heat transfer problems 
•  Keyword  family:  *MESH_,  the  keywords  starting  with  *MESH  refer  to  and 
control  the  tools  for  the  automatic  volume  mesh  generator  for  the  CESE  and 
ICFD solvers. 
◦  Mesh Generator Characteristics: 
  Automatic 
  Robust 
  Generic 
  Tetrahedral elements for 3D, Triangles in 2D 
  Closed body fitted mesh (surface mesh) needs to be provided for vol-
ume generation 
◦  Mesh Generator Main Features: 
  Automatic  remeshing  to  keep  acceptable  mesh  quality  for  FSI  prob-
lems (ICFD only) 
  Adaptive meshing tools (ICFD only) 
  Anisotropic boundary layer mesh 
  Mesh element size control tools 
  Remeshing tools for surface meshes to ensure mesh quality 
◦  Mesh Generator Applications : 
  Used by the Incompressible CFD solver (ICFD).   
  Used by the Compressible CFD solver (CESE). 
Other additions to Version 7 include: 
•  Add  new  parameter  VNTOPT  to  *AIRBAG_HYBRID,  that  allows  user  more 
control on bag venting area calculation. 
•  Allow  heat  convection  between  environment  and  CPM  bag  (*AIRBAG_PARTI-
CLE)  bag.    Apply  proper  probability  density  function  to  part's  temperature 
created by the particle impact. 
•  *AIRBAG_PARTICLE  and  *SENSOR_SWITCH_SHELL_TO_VENT  allows  user 
to  input  load  curve  to  control  the  venting  using  choking  flow  equation  to  get 
proper  probability  function  for  vents.    Therefore,  this  vent  will  have  the  same 
vent rate as real vent hole.
INTRODUCTION 
•  Add new option NP2P in *CONTROL_CPM to control the repartition frequency 
of CPM particles among processors (MPP only). 
•  Enhance  *AIRBAG_PARTICLE  to  support  a  negative  friction  factor  (FRIC  or 
PFRIC) in particle to fabric contact.  Particles are thus able to rebound at a trajec-
tory closer to the fabric surface after contact. 
•  Use  heat  convection  coefficient  HCONV  and  fabric  thermal  conductivity  KP  to 
get  correct  effective  heat  transfer  coefficient  for  heat  loss  calculation  in 
*AIRBAG_PARTICLE.  If KP is not given, H will be used as effective heat trans-
fer coefficient. 
•  Extend CPM inflator orifice limit from 100 to unlimited (*AIRBAG_PARTICLE). 
•  Support  dm_in_dt  and  dm_out_dt  output  to  CPM  chamber  database  (*DATA-
BASE_ABSTAT)  to  allow  user  to  study  mass  flow  rate  between  multiple  cham-
bers. 
•  Previously,  the  number  of  ships  (rigid  bodies)  in  *BOUNDARY_MCOL,  as 
specified  by  NMCOL,  was  limited  to  2.   Apparently, this  was  because  the  code 
had  not  been  validated  for  more  than  2  rigid  bodies,  but  it  is  believed  that  it 
should not be a problem to remove this restriction.  Consequently, this limit has 
been raised to 10, with the caveat that the user should verify the results for NM-
COL > 2. 
a 
•  Implemented 
structural-acoustic  mapping 
(*BOUNDARY_-
ACOUSTIC_MAPPING),  for  mapping  transient  structural  nodal  velocity  to 
acoustic volume surface nodes.  This is useful if the structure finite element mesh 
and the acoustic boundary/finite element mesh are mismatched. 
scheme 
•  *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURACE_ORTHO_FRIC-
TION  can  now  be  defined  by  part  set  IDs  when  supplemented  by  *DEFINE_-
FRICTION_ORIENTATION.  Segment sets with orientation per *DEFINE_FRIC-
TION_ORIENTATION are generated automatically. 
•  Contact force of *CONTACT_ENTITY is now available in intfor (*DATABASE_-
BINARY_INTFOR). 
•  *CONTACT_FORCE_TRANSDUCER_PENALTY  will  now  accept  node  sets  for 
both the slave and master sides, which should allow them to work correctly for 
eroding materials.  BOTH sides should use node sets, or neither. 
•  Added  option  to  create  a  backup  penalty-based  contact  for  a  tied  constraint-
based contact in the input (IPBACK on Card E of *CONTACT). 
•  New  option  for  *CONTACT_ENTITY.    If  variable  SO  is  set  to  2,  then  a  con-
straint-like option is used to compute the forces in the normal direction.  Friction 
is treated in the usual way. 
•  *CONTACT_ENTITY:  allow  friction  coefficient  to  be  given  by  a  “coefficient  vs 
time” load curve (input < 0 -> absolute value is the load curve ID).  Also, if the 
friction coefficient bigger or equal 1.0, the node sticks with no sliding at all.
INTRODUCTION 
•  Minor tweak to the way both MPP and SMP handle nodes sliding off the ends of 
beams in *CONTACT_GUIDED_CABLE. 
•  Frictional energy output in sleout (*DATABASE_SLEOUT) supported for *CON-
TACT_…_MORTAR. 
•  Tiebreak  damage  parameter  output  as  “contact  gap”  in  intfor  file  for  *CON-
OP-
TACT_AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK_MORTAR, 
TION = 9. 
•  Added  MPP  support  for  *CONTACT_2D_AUTOMATIC_SINGLE_SURFACE 
and *CONTACT_2D_AUTOMATIC_SURFACE_TO_SURFACE. 
•  Added  keyword  *CONSTRAINED_MULTIPLE_GLOBAL  for  defining  multi-
node constraints for imposing periodic boundary conditions.   
•  Enhancement  for  *CONSTRAINED_INTERPOLATION_SPOTWELD  (SPR3): 
calculation of bending moment is more accurate now. 
•  If  *CONSTRAINED_NODAL_RIGID_BODY  nodes  are  shared  by  several 
processors  with  mass  scaling  on,  the  added  mass  is  not  summed  up  across 
processors.  This results in an instability of the NRB.  (MPP only) 
•  *ALE_REFINE  has  been  replaced  and  expanded  upon  by  the  *CONTROL_RE-
FINE  family  of  commands.    These  commands  invoke  local  mesh  refinement  of 
shells, solids, and ALE elements based on various criteria. 
•  Shells or solids in a region selected for refinement (parent element) are replaced 
by  4  shells  or  8  solids,  respectively.    *CONTROL_REFINE_SHELL  applies  to 
shells,  *CONTROL_REFINE_SOLID  applies  to  solids  and  *CONTROL_RE-
FINE_ALE  and  *CONTROL_REFINE_ALE2D  applies  to  ALE  elements.    Each 
keyword has up to 3 lines of input.  If only the 1st card is defined, the refinement 
occurs  during  the  initialization.    The  2nd  card  defines  a  criterion  CRITRF  to 
automatically refine the elements during the run.  If the 3rd card is defined, the 
refinement  can  be  reversed  based  on  a  criterion  CRITM.    All  commands  are 
implemented for MPP. 
•  *CONTROL_REFINE_MPP_DISTRIBUTION  distributes  the  elements  required 
by the refinement across the MPP processes. 
•  Eliminate  automatic  writing  of  a  d3plot  plot  state  after  each  3D  tetrahedral 
remeshing operation (*CONTROL_REMESHING) to reduce volume of output. 
•  Generate  disbout  output  (*DATABASE_DISBOUT)  for  MPP  and  SMP  binout 
files. 
•  Extend  *DATABASE_MASSOUT  to  include  option  to  output  mass  information 
on rigid body nodes. 
•  Added  new  keyword  *CHANGE_OUTPUT  for  full  deck  restart  to  override 
default behavior of overwriting existing ASCII files.  For small restart, this option
INTRODUCTION 
has  no  effect  since  all  ASCII  output  is  appended  to  the  result  of  previous  run 
already. 
•  Added new option (NEWLENGD) to 2nd field of 3rd card of *CONTROL_OUT-
PUT to write more detailed legend in ASCII output files.  At present, only rcforc 
and jntforc are implemented. 
•  Increased default binary file size scale factor (x=) from 7 to 1024.  That means the 
default binary file size will be 1  Gb  for single version and 2 Gb for double ver-
sion. 
•  Add echo of new “max frequency of element failure summaries” flag (FRFREQ 
in *CONTROL_OUTPUT) to d3hsp file. 
•  Support  LSDA/binout  output  for  new  pllyout  file  (*DATABASE_PLLYOUT, 
*ELEMENT_BEAM_PULLEY) in both SMP and MPP. 
•  Allow  degenerated  hexahedrons 
for  cohesive  solid  elements 
(ELFORM = 19, 20) that evolve from an extrusion of triangular shells.  The input 
of  nodes  on  the  element  cards  for  such  a  pentahedron  is  given  by:  N1,  N2,  N3, 
N3, N4, N5, N6, N6. 
(pentas) 
•  Add  new  option  to  activate  drilling  constraint  force  for  shells  in  explicit 
calculations.    This  can  be  defined  by  parameters  DRCPSID  (part  set)  and  DR-
CPRM (scaling factor) on *CONTROL_SHELL. 
•  Add SMP ASCII database “pllyout” (*DATABASE_PLLYOUT) for *ELEMENT_-
BEAM_PULLEY. 
•  *FREQUENCY_DOMAIN_ACOUSTIC_BEM: 
◦  Added an option to output real part of acoustic pressure in time domain. 
◦  Enabled BEM acoustic computation following implicit transient analysis. 
◦  Implemented  coupling  between  steady  state  dynamics  and  collocation 
acoustic BEM. 
◦  Implemented  Acoustic  Transfer  Vector  (ATV)  to  variational  indirect  BEM 
acoustics. 
◦  Enabled boundary acoustic mapping in BEM acoustics. 
•  *FREQUENCY_DOMAIN_ACOUSTIC_FEM: 
◦  Added boundary nodal velocity to binary plot file d3acs. 
◦  Implemented pentahedron elements in FEM acoustics. 
◦  Enabled using boundary acoustic mapping in FEM acoustics. 
•  *FREQUENCY_DOMAIN_FRF: 
◦  Updated FRF to include output in all directions (VAD2 = 4). 
◦  Added treatment for FRF with base acceleration (node id can be 0).
INTRODUCTION 
•  *FREQUENCY_DOMAIN_RANDOM_VIBRATION: 
◦  Updated calculation of PSD and RMS von Mises stress in random vibration 
environment, based on Sandia National Laboratories report, 1998. 
•  *FREQUENCY_DOMAIN_RANDOM_VIBRATION_FATIGUE: 
◦  Implemented  an  option  to  incorporate  initial  damage  ratio  in  random  vi-
bration fatigue. 
•  *FREQUENCY_DOMAIN_RESPONSE_SPECTRUM: 
◦  Implemented  double  sum  methods  (based  on  Gupta-Cordero  coefficient, 
modified Gupta-Cordero coefficient, and Rosenblueth-Elorduy coefficient). 
◦  Updated calculating von Mises stress in response spectrum analysis. 
◦  Implemented treatment for multi simultaneous input spectra. 
◦  Improved double sum methods by reducing number of loops. 
•  *FREQUENCY_DOMAIN_SSD: 
◦  Added  the  option  to  output  real  and  imaginary  parts  of  frequency  re-
sponse to d3ssd. 
◦  Added  the  option  to  output  relative  displacement,  velocity  and  accelera-
tion in SSD computation in the case of base acceleration.  Previously only 
absolute values were provided. 
•  Implemented  keyword  *FREQUENCY_DOMAIN_MODE_{OPTION}  so  that 
user can select the vibration modes to be used for frequency response analysis. 
•  Implemented  keyword  *SET_MODE_{OPTION}  so  that  user  can  define  a  set  of 
vibration modes, to be used for frequency response analysis. 
•  Implemented  keyword  *FREQUENCY_DOMAIN_PATH  to  define  the  path  of 
binary  databases  containing  mode  information,  used  in  restarting  frequency 
domain analysis, e.g.  frf, ssd, random vibration. 
•  Compute normal component of impulse for oblique plates in *INITIAL_MINE_-
IMPULSE.  The feature is no longer limited to horizontal plates. 
•  Disable license security for *INITIAL_IMPULSE_MINE.  The feature is no longer 
restricted. 
•  Enabled  hourglass  type  7  to  work  well  with  *INITIAL_FOAM_REFERENCE_-
GEOMETRY so that initial hourglass energy is properly calculated and foam will 
spring back to the initial geometry. 
•  Accommodate erosion of thin shells in *LOAD_BLAST_ENHANCHED.
INTRODUCTION 
•  *LOAD_VOLUME_LOSS  has  been  changed  such  that  after  the  analysis  time 
exceeds  the  last  point  on  the  curve  of  volume  change  fraction  versus  time,  the 
volume change is no longer enforced. 
•  *LOAD_BODY_POROUS  new  option  AOPT  added  to  assign  porosity  values  in 
material coordinate system. 
•  Added *LOAD_SEGMENT_FILE. 
•  Add  new  sensor  definition,  *SENSOR_DEFINE_ANGLE.    This  card  traces  the 
angle formed between two lines. 
•  *SENSOR_DEFINE_NODE  can  be  used  to  trace  the  magnitude  of  nodal  values 
(coordinate, velocity or accleration) when VID is “0” or undefined. 
•  Add  two  new  parameters  to  *SENSOR_DEFINE_ELEMENT,  scale  factor  and 
power,  so  that  user  can  adjust  the  element-based  sensor  values  (strain,  stress, 
force, …). 
•  Change  history  variables  10-12  in  *MAT_054/*MAT_ENHANCED_COMPOS-
ITE_DAMAGE  (thin  shells  only)  to  represent  strains  in  material  coordinate 
system rather than in local element coordinate system.  This is a lot more helpful 
for postprocessing issues.  This change should not lead to different results other 
than due to different round-off errors. 
•  New features and enhancements to *MAT_244/*_MAT_UHS_STEEL: 
◦  Added implicit support for MAT_244. 
◦  Changed the influence of the austenite grain size in Mat244 according to Li 
et al. 
◦  Changed the start temperatures to fully follow WATT et al and Li et al. 
◦  Hardness calculation is now improved when noncontinuous cooling is ap-
plied i.e., tempering. 
◦  Added temperature dependent Poisson ratio and advanced reaction kinet-
ics. 
◦  Added  new  advanced  option  to  describe  the  thermal  expansion  coeffi-
cients for each phase. 
◦  Added option to use Curve ID or a Table ID for describing the latent heat 
generation during phase transormations. 
◦  Added  support  for  table  definition  for  Youngs  modulus.    Now  you  can 
have one temperature dependent curve for each of the 5 phases 
•  Added support for implicit to *MAT_188. 
•  Added  material  model  *MAT_273/*MAT_CDPM/*MAT_CONCRETE_DAM-
AGE_PLASTIC_MODEL.    This  model  is  aimed  at  simulations  where  failure  of 
concrete structures subjected to dynamic loadings is sought.  The model is based 
on effective stress plasticity and has a damage model based on both plastic and 
elastic  strain  measures.    Implemented  for  solids  only  but  both  for  explicit  and
INTRODUCTION 
implicit simulations.  Using an implicit solution when damage is activated may 
trigger a slow convergense.  IMFLAG = 4 or 5 can be useful. 
•  Added an option in *MAT_266 (*MAT_TISSUE_DISPERSED) so that the user can 
tailor the active contribution with a time dependent load curve instead of using 
the internal hardcoded option.  See ACT10 in the User's Manual. 
•  *MAT_173/*MAT_MOHR_COULOMB is available in 2D. 
•  Enable  *MAT_103  and  *MAT_104  to  discretize  the  material  load  curves  accord-
ing to the number of points specified by LCINT in *CONTROL_SOLUTION. 
•  Implement Prony series up to 18 terms for shells using *MAT_076/*MAT_GEN-
ERAL_VISCOELASTIC. 
•  Added *DEFINE_STOCHASTIC_VARIATION and the STOCHASTIC option for 
*MATs 10, 15, 24, 81, 98 for shells, solids, and type 13 tets.  This feature defines a 
stochastic variation in the yield stress and damage/failure of the aforementioned 
material models. 
•  Add  Moodification  for  *DEFINE_CONNECTION_PROPERTIES,  PROPRUL = 2: 
thinner weld partner is first partner, PROPRUL = 3: bottom (nodes 1-2-3-4) weld 
partner is first partner. 
•  Add spotweld area to debug output of *DEFINE_CONNECTION_PROPERTIES 
which is activated by *CONTROL_DEBUG. 
•  Add  support  of  *MAT_ADD_EROSION  option  NUMFIP < 0  for  standard  (non-
GISSMO) failure criteria.  Only for shells. 
•  Improve  implicit  convergence  of  *MAT_ADD_EROSION  damage  model  GISS-
MO by adding damage scaling (1-D) to the tangent stiffness matrix. 
•  Provide  plastic  strain  rates  (tension/compression,  shear,  biaxial)  as  history 
variables no.  16, 17, and 18 for *MAT_187. 
•  Add  new  variables  to  user  failure  routine  matusr_24  (activated  by  FAIL < 0  on 
*MAT_024 and other materials): integration point numbers and element id. 
•  Add  new  energy  based,  nonlocal  failure  criterion  for  *MAT_ADD_EROSION, 
parameters  ENGCRT  (critical  energy)  and  RADCRT  (critical  radius)  after  EP-
STHIN.  Total internal energy of elements within a radius RADCRT must exceed 
ENGCRT for erosion to occur.  Intended for windshield impact. 
•  Add  new  option  to  *MAT_054  for  thin  shells:  Load  curves  for  rate  dependent 
strengths and a rate averaging flag can be defined on new optional card 9. 
•  Add new option for *MAT_MUSCLE: Input parameter SSP < 0 can now refer to a 
load curve (stress vs.  stretch ratio) or a table (stress vs.  stretch ratio vs.  normal-
ized strain rate). 
•  Expand  list  of  variables  for  *MAT_USER_DEFINED_MATERIAL_MODELS  by 
characteristic element size and element id.
INTRODUCTION 
•  Enable 
*MAT_USER_DEFINED_MATERIAL_MODELS 
tetrahedron  element  type  13. 
“umat41v_t13” show corresponding pressure calculation in the elastic case. 
to  be  used  with 
  New  sample  routines  “umat41_t13”  and 
•  Add a new feature to *MAT_125 allowing C1 and C2 to be used in calculation of 
back  stress.    When  plastic  strain < 0.5%,  C1  is  used,  otherwise  C2  is  used  as 
described in Yoshida's paper. 
•  Extend non-linear strain path (_NLP_FAILURE) in *MAT_037 to implicit. 
•  *MAT_173/*MAT_MOHR_COULOMB  now  works  in  ALE.    A  new  option  has 
been added to suppress the tensile limit on hydrostatic stress recommended for 
ALE multi-material use. 
•  Upgraded *MAT_172/*MAT_CONCRETE_EC2. 
◦  Corrections to DEGRAD option. 
◦  Concrete  and  reinforcement  types  7  and  8  have  been  added  to  reflect 
changes to Eurocode 2. 
◦  Extra history variables for reinforcement stress and strain are now output 
as zero for zero-fraction reinforcement directions. 
•  Added RCDC model for solid *MAT_082. 
•  Added Feng's failure model to solid *MAT_021. 
•  Added *MAT_027 for beams. 
•  Added *DEFINE_HAZ_PROPERTIES and *DEFINE_HAZ_TAILOR_WELDED_-
BLANK for modifying material behavior near a spot weld. 
•  Added fourth rate form to viscoplastic Johnson-Cook model (*MAT_015). 
•  Added option to *MAT_224 to not delete the element if NUMINT = -200. 
•  New  damage  initiation  option  3  in  multi  fold  damage  criteria  in  *MAT_ADD_-
EROSION.  Very similar to option 2 but insensitive to pressure. 
•  Added  rotational  resistance  in  *MAT_034/*MAT_FABRIC.    Optionally  the  user 
may  specify  the  stiffness,  yield  and  thickness  of  and  elastic-perfectly-plastic 
coated layer of a fabric that results in a rotational resistance during the simula-
tion. 
•  FLDNIPF < 0  in  *MAT_190/*MAT_FLD_3-PARAMETER_BARLAT  for  shell 
elements means that failure occurs when all integration points within a relative 
distance of -FLDNIPF from the mid surface has reached the fld criterion. 
•  A  computational  welding  mechanics  *MAT_270/*MAT_CWM  material  is 
available  that  allows  for  element  birth  based  on  a  birth  temperature  as  well  as 
annealing  based  on  an  annealing  temperature.    The  material  is  in  addition  a 
thermo-elasto-plastic  material  with  kinematic  hardening  and  temperature  de-
pendent properties.
INTRODUCTION 
•  Added  *MAT_271/*MAT_POWDER,  a  material 
(i.e., 
compaction  and  sintering)  of  cemented  carbides.    It  is  divided  into  an  elastic-
plastic compaction model that is supposed to be run in a first phase, and a visco-
elastic sintering model that should be run in a second phase.  This model is for 
solid elements. 
for  manufacturing 
•  For IHYPER = 3 on a *MAT_USER_DEFINED_… shell material, the deformation 
gradient is calculated from the geometry instead of incremented by the velocity 
gradient.    The  deformation  gradient  is  also  passed  to  the  user  defined  subrou-
tines  in  the  global  system  together  with  a  transformation  matrix  between  the 
global  and  material  frames.    This  allows  for  freedom  in  how  to  deal  with  the 
deformation gradient and its transformations in orthotropic (layered) materials. 
•  The Bergstrom-Boyce viscoelastic rubber model is now available in explicit and 
implicit  analysis  as  *MAT_269/*MAT_BERGSTROM_BOYCE_RUBBER.    The 
Arruda-Boyce  elastic  stress  is  augmented  with  a  Bergstrom-Boyce  viscoelastic 
stress corresponding to the response of a single entangled chain in a polymer gel 
matrix. 
•  Added  a  new  parameter  IEVTS  to  *MAT_USER_DEFINED_MATERIAL_MOD-
ELS (*MAT_041-050).  IEVTS is optional and is used only by thick shell formula-
tion 5.  It points to the position of E(a) in the material constants array.  Following 
E(a), the next 5 material constants must be E(b), E(c), v(ba), v(ca), and v(cb).  This 
data  enables  thick  shell  formulation  5  to  calculate  an  accurate  thickness  strain, 
otherwise the thickness strain will be based on the elastic constants pointed to by 
IBULK and IG. 
•  Implemented enhancements to fabric material (*MAT_034), FORM = 14.  Stress-
strain  curves  may  include  a  portion  for  fibers  in  compression.    When  un-
load/reload curves with negative curve ID are input (curve stretch options), the 
code  that  finds  the  intersection  point  now  extrapolates  the  curves  at  their  end 
rather  than  simply  printing  an  error  message  if  an  intersection  point  cannot  be 
found before the last point in either curve. 
•  Map  1D  to  3D  by  beam-volume  averaging  the  1D  data  over  the  3D  elements 
(*INITIAL_ALE_MAPPING). 
•  In a 3D to 3D mapping (*INITIAL_ALE_MAPPING),  map the relative displace-
ments for the penalty coupling in *CONSTRAINED_LAGRANGE_IN_SOLID. 
•  The  [name].xy  files  associated  with  *DATABASE_ALE_MAT  are  now  created 
when sense switches sw1, sw2, quit, or stop are issued. 
•  *ALE_ESSENTIAL_BOUNDARY is available in 2D. 
•  *DATABASE_FSI is available for 2D (MPP). 
•  *ALE_ESSENTIAL_BOUNDARY  implemented  to  apply  slip-only  velocity  BC 
along ALE mesh surface.
INTRODUCTION 
•  *CONTROL_ALE flag INIJWL = 2 option added to balance initial pressure state 
between ALE Soil and HE. 
•  Include SPH element (*ELEMENT_SPH) in time step report. 
•  Time step and internal energy of 2D axisymmetric SPH elements  are calculated 
in a new way more consistent with the viscosity force calculation. 
•  Only  apply  viscosity  force  to  x  and  y  components  of  2D  axisymmetric  SPH 
element, not on hoop component. 
•  MAXV  in  *CONTROL_SPH  can  be  defined  as  a  negative  number  to  turn  off 
velocity checking. 
•  Improve  calculation  of  2D  axisymmetric  SPH  contact  force  in  *DEFINE_SPH_-
TO_SPH_COUPLING. 
•  Added  the  following  material  models  for  SPH  particles:  *MAT_004/*MAT_-
ELASTIC_PLASTIC_THERMAL  (3D  only)  and  *MAT_106/*MAT_ELASTIC_-
VISCOPLASTIC_THERMAL 
•  Added  a  new  parameter  DFACT  for  *DEFINE_SPH_TO_SPH_COUPLING.  
DFACT  invokes  a  viscous  term  to  damp  the  coupling  between  two  SPH  parts 
and thereby reduce the relative velocity between the parts. 
•  Added  BOUNDARY_CONVECTION  and  BOUNDARY_RADIATION 
for 
explicit SPH thermal solver. 
•  *CONTROL_REMESHING_EFG: 
◦  Add  eroding  failed  surface  elements  and  reconstructing  surface  in  EFG 
adaptivity. 
◦  Add a control parameter for monotonic mesh resizing in EFG adaptivity. 
◦  Add searching and correcting self-penetration for adaptive parts in 3D tet-
rahedron remeshing. 
•  Enhance 3D axisymmetric remeshing with 6-node/8-node elements  
•  (*CONTROL_REMESHING): 
◦  Use RMIN/RMAX along with SEGANG to determine element size. 
◦  Remove the restriction that the reference point of computational model has 
to be at original point (0, 0, 0). 
◦  Rewrite  the  searching  algorithm  for  identifying  the  feature  lines  of  cross-
sections in order to provide more stable remeshing results. 
•  Improve rigid body motion in EFG shell type 41. 
•  Support EFG pressure smoothing in EFG solid type 42 for *MAT_ELASTIC_VIS-
COPLASTIC_THERMAL. 
•  Add visco effect for implicit EFG solid type 42.
INTRODUCTION 
•  Add  new  EFG  solid  type  43  (called  Meshfree-Enriched  FEM,  MEFEM)  for  both 
implicit and explicit.  This element formulation is able to relieve the volumetric 
locking  for  nearly-incompressible  material  (eg.    rubber)  and  performs  strain 
smoothing across elements with common faces. 
•  EFG shell adaptivity no longer requires a special license. 
•  Application of EFG in an implicit analysis no longer requires a special license. 
•  Add *SENSOR_CONTROL for prescribed motion constraints in implicit. 
•  Update  *INTERFACE_LINKING_NODE  in  implicit  to  catch  up  with  explicit, 
including adding scaling factors. 
•  Add support for *DATABASE_RCFORC_MOMENT for implicit. 
•  Enhance Iterative solvers for Implicit Mechanics. 
•  Add, after the first implicit time step, the output of projected cpu and wall clock 
times.  This was already in place for explicit.  Also echo the termination time. 
•  Add  variable  MXDMP  in  *CONTROL_THERMAL_SOLVER  to  write  thermal 
conductance matrix and right-hand side every MXDMP time steps. 
•  Add  keyword  *CONTROL_THERMAL_EIGENVALUE  to  calculate  eigenval-
ue(s) of each thermal conductance matrix. 
•  Added  thermal  material  model  *MAT_THERMAL_ORTHOTROPIC_TD_LC.  
This is an orthtropic material with temperature dependent properties defined by 
load curves. 
•  Changed  structured  file  format  for  control  card  27  (first  thermal  control  card).  
Several  input  variables  used  i5  format  limiting  their  value  to  99,999.    A  recent 
large model exceeded this limit.  The format was changed to i10.  This change is 
not  backward  compatible.    Old  structured  input  files  will  no  longer  run  unless 
control card 27 is changed to the new i10 format.  This change does not affect the 
KEYWORD file. 
•  Add 
thermal  material  *MAT_T07/*MAT_THERMAL_CWM 
for  welding 
simulations,  to  be  used  in  conjunction  with  mechanical  counterpart  *MAT_-
270/*MAT_CWM. 
•  Modify decomposition costs of *MAT_181 and *MAT_183. 
•  Introduce new timing routines and summary at termination. 
•  Echo “MPP contact is groupable” flag to d3hsp 
•  Bodies using *MAT_RIGID_DISCRETE were never expected to share nodes with 
non-rigid bodies, but this now works in MPP. 
•  There is no longer any built-in limitation on the number of processors that may 
be used in MPP.
INTRODUCTION 
•  Echo contents of the MPP pfile (including keyword additions) to the d3hsp and 
mes0000 files. 
•  Add  new  keyword  *CONTROL_MPP_PFILE,  which  allows  for  insertion  of  text 
following this command to be inserted into the MPP pfile (p = pfile). 
•  Change in MPP treatment of *CONSTRAINED_TIE-BREAK.  They now share a 
single  MPI  communicator,  and  a  single  round  of  communication.    This  should 
improve performance for problems with large numbers of these, without affect-
ing the results. 
•  Added  two  input  variables  for  *CONTROL_FORMING_ONESTEP  simulation, 
TSCLMIN is a scale factor limiting the thickness reduction and EPSMAX defines 
the maximum plastic strain allowed. 
•  Added output of strain and stress tensors for onestep solver *CONTROL_FORM-
ING_ONESTEP, to allow better evaluation of formability. 
•  Improved *CONTACT_AUTO_MOVE: before changes the termination time, and 
it causes problems when several tools need to be moved.  Now *CONTACT_AU-
TO_MOVE does not change the termination time, but changes the current time.  
In  this  way,  several  tools  can  be  moved  without  the  need  to  worry  about  the 
other  tool's  move.    This  is  especially  useful  in  multi-flanging  and  hemming 
simulations. 
•  Made  improvements  to  previously  undocumented  keyword  *INTERFACE_-
BLANKSIZE,  including  adding  the  options_INITIAL_TRIM,  and_INITIAL_-
ADAPTIVE.  This keyword was developed for blank size development in sheet 
metal forming.  Generally, for a single forming process, only the option_DEVEL-
OPMENT  is  needed  and  inputs  are  an  initial  estimated  blank  shape,  a  formed 
blank  shape,  and  a  target  blank  shape  in  either  mesh  or  boundary  coordinates.  
Output  will  be  the  calculated/corrected  initial  blank  shape.    Initial  blank  mesh 
and  formed  blank  mesh  can  be  different  (e.g.    adaptive).    For  a multi-stamping 
process  involving  draw,  trimming  and  flanging,  all  three  options  are  needed.  
Related  commands  for  blank  size  estimation  are  *CONTROL_FORMING_ON-
ESTEP, and for trim line development, *CONTROL_FORMING_UNFLANGING. 
•  Made improvements and added features to previously undocumented keyword 
*CONTROL_FORMING_UNFLANGING,  this  keyword  unfolds  flanges  of  a 
deformable blank, e.g., flanged or hemmed portions of a sheet metal part, onto a 
rigid tooling mesh using the implicit static solver.  It is typically used in trim line 
mapping  during  a  draw  die  development  process.    The  roots  of  the  flanges  or 
hemmed edges are automatically processed based on a  user input  of a distance 
tolerance  between  the  flanges/hemmed  edges  and  rigid  tool.    It  includes  the 
ability  to  handle  a  vertical  flange  wall.    Other  keywords  related  to  blank  size 
development  are,  *CONTROL_FORMING_ONESTEP,  and  *INTERFACE_-
BLANKSIZE_DEVELOPMENT.
INTRODUCTION 
•  Added  keyword  *CONTROL_FORMING_OUTPUT  which  allows  control  of 
d3plot output by specifying distances to tooling home.  It works with automatic 
position of stamping tools using *CONTROL_FORMING_AUTOPOSITION_PA-
RAMETER. 
•  Added the LOCAL_SMOOTH option to *INTERFACE_COMPENSATION_NEW 
which  features  smoothing  of  a  tool's  local  area  mesh,  which  could  otherwise 
become  distorted  due  to,  e.g.,  bad/coarse  mesh  of  the  original  tool  surface, 
tooling  pairs  (for  example,  flanging  post  and  flanging  steel)  do  not  maintain  a 
constant gap and several compensation iterations.  This new option also allows 
for  multiple  regions  to  be  smoothed.    Local  areas  are  defined  by  *SET_LIST_-
NODE_SMOOTH. 
•  Added output to rcforc for *DEFINE_DE_TO_SURFACE_COUPLING. 
•  Implement traction surface for *DEFINE_DE_TO_SURFACE_COUPLING. 
•  Add  keyword  *DATABASE_BINARY_DEMFOR  with  command  line  option 
dem = dem_int_force.    This  will  turn  on  the  DEM  interface  force  file  for  DEM 
coupling option.  The output frequency is controlled by the new keyword. 
•  Add  new  feature  *DEFINE_DE_INJECTION  to  allow  DEM  particle  dropping 
from user defined plane. 
•  Add new option_VOLUME to *ELEMENT_DISCRETE_SPHERE.  This will allow 
DEM  input  based  on  per  unit  density  and  use  *MAT  card  to  get  consistent 
material properties. 
•  Added  FORM = -4  for  *ELEMENT_SHELL_NURBS_PATCH.    Rotational  dofs 
are  automatically  set  at  control  points  at  the  patch  boundaries,  whereas  in  the 
interior  of  the  patch  only  translational  dofs  are  present.    This  helps  for  joining 
multiple nurbs patches at their C0-boundaries. 
•  Disabled  FORM = 2  and  3  for  *ELEMENT_SHELL_NURBS_PATCH.    These 
formulations are experimental and not fully validated yet. 
•  Added  energy  computation  for  isogeometric  shells  (*ELEMENT_SHELL_-
NURBS_PATCH) to matsum. 
•  Allow  isogeometric  shells  (*ELEMENT_SHELL_NURBS_PATCH)  to  behave  as 
rigid body (*MAT_RIGID). 
•  Added  “g”  as  abbreviation  for  gigawords  in  specification  of  memory  on 
execution line, e.g, memory = 16g is 16 billion words. 
•  Suppress non-printing characters in *COMMENT output. 
•  Add command line option “pgpkey” to output the current public PGP key used 
by  LS-DYNA.    The  output  goes  to  the  screen  as  well  as  a  file  named  “lstc_
pgpkey.asc” suitable for directly importing into GPG.
INTRODUCTION 
•  When reading the NAMES file, allow a “+” anywhere on a line to indicate there 
will be a following line, not just at the end.  This was never intended, but worked 
before r73972 and some customers use it that way. 
•  Check  for  integer  overflow  when  processing  command  line  arguments  and  the 
memory value on the *KEYWORD card. 
•  Added  new  capability  for  *INTERFACE_LINKING_NODE  to  scale  the  dis-
placements of the moving interface. 
•  Support for *KEYWORD_JOBID with internal *CASE driver. 
•  *DAMPING_FREQUENCY_RANGE  now  works  for  implicit  dynamic  solutions.  
An  error  check  has  been  added  to  ensure that  the  timestep  is  small  enough  for 
the damping card to work correctly. 
•  Added  new  option  *DAMPING_FREQUENCY_RANGE_DEFORM  to  damp 
only the deformation instead of the global motion. 
•  Added *DEFINE_VECTOR_NODES.  A vector is defined using two node IDs. 
•  Add sense switch “prof” to output current timing profile to message (SMP) file 
or  mes####  (MPP)  files.    Also,  for  MPP  only,  collect  timing  information  from 
processor and output to prof.out when sense switch “prof” is detected.   
Capabilities added during 2013/2014 to create LS-DYNA R7.1:  
•  Add  MUTABLE  option  for  *PARAMETER  so  that  parameter  values  can  be 
redefined later in the input deck. 
•  Change  MPP  treatment  of  two-sided  *CONTACT_FORCE_TRANSDUCER  so 
that proper mass and moment values can be output to the rcforc file. 
•  MPP support for non-zero birthtime for *CONTACT_SINGLE_EDGE. 
•  Add  new  command  line  option  “ldir=”  for  setting  a local  working directory.   In 
MPP, this has the same effect as setting the “directory { local }” pfile option (and 
it overrides that option).  For SMP, it indicates a directory where local, working 
files should be placed. 
•  Add support for SMOOTH option in MPP groupable contact. 
•  Add  new  keyword  card  *CONTROL_REQUIRE_REVISION  to  prevent  the 
model from being run in old versions of LS-DYNA. 
•  Add  part  set  specification  for  dynamic  relaxation  with  implicit  using  *CON-
TROL_DYNAMIC_RELAXATION. 
  This  is  a  new  feature  specified  with 
idrflg = 6 on *CONTROL_DYNAMIC_RELAXATION.  This allows implicit to be 
used for the dynamic relaxation phase for models involving parts being modeled 
with SPH and/or ALE while excluding those parts from the dynamic relaxation 
phase.
INTRODUCTION 
•  Add  new  feature  for  implicit  automatic  time  step  control  to  cooperate  with 
thermal time step control.  On *CONTROL_IMPLICIT_AUTO, IAUTO = 2 is the 
same as IAUTO = 1 with the extension that the implicit  mechanical time step is 
limited by the active thermal time step. 
•  On  *CONTROL_IMPLICIT_SOLUTION,  add  negative  value  of  MAXREF  for 
implicit  mechanics.    Nonlinear  iteration  will  terminate  after  |MAXREF|  itera-
tions.    With  MAXREF < 0  convergence  is  declared  with  a  warning.    Simulation 
will continue.  Positive values of MAXREF still cause failure of convergence to be 
declared leading to either a time step reduction or an error termination. 
•  Add *CONTROL_IMPLICIT_MODAL_DYNAMIC keywords and features.  This 
elevates  the  modal  dynamic  features  of  IMASS = 2  on  *CONTROL_IMPLICIT_-
DYNAMICS.    It  also  adds  additional  features  of  damping  and  mode  selection 
and stress computations. 
•  New  material  model  *MAT_DRY_FABRIC  /  MAT_214,  which  can  be  used  in 
modeling high strength woven fabrics with transverse orthotropic behavior. 
•  Add  *ALE_COUPLING_NODAL_PENALTY,  penalty-based  nodal  coupling 
with ALE. 
•  Add  type  8  *ELEMENT_SEATBELT_PRETENSIONER  which  takes  energy-time 
curve, instead of pull-in or force curve. 
•  Add type 9 *ELEMENT_SEATBELT_PRETENSIONER for energy-based buckle / 
anchor pretensioner. 
•  Add  *DATABASE_BINARY_FSILNK.    This  feature  stores  coupling  pressure 
from *CONSTRAINED_LAGRANGE_IN_SOLID in a binary time history file for 
use in a separate model that does not include ALE. 
•  Add *LOAD_SEGMENT_FSILNK.  Use pressure loads stored in aforementioned 
binary time history file to load model that does not have ALE elements. 
•  Add  new  keyword  *DEFINE_SPH_DE_COUPLING  to  allow  SPH  particles  to 
contact discrete element spheres (DES). 
•  Add  MOISTURE  option  to  *MAT_076  solids.    Allows  moisture  content  to  be 
input as a function of time.  Material parameters are then scaled according to the 
moisture and a moisture strain is also introduced. 
•  Add  *RIGIDWALL_FORCE_TRANSDUCER  to  output  forces  from  rigidwalls 
acting on node sets. 
•  Add  LOG_INTERPOLATION  option  to  *MAT_024.    This  offers  an  alternate 
means  of  invoking  logarithmic  interpolation  for  strain  rate  effects.    The  other 
way is to input the natural log of strain rate in the table LCSS. 
•  Add capability in *MAT_ADD_EROSION (NUMFIP < -100) to set stress to zero 
in  each  shell  integration  point  as  it  reaches  the  failure  criterion.    When 
|NUMFIP|-100  integration  points  have  failed,  the  shell  is  eroded.    In  contrast,
INTRODUCTION 
when NUMFIP > 0, failed integration points continue to carry full load as though 
they were unfailed until element erosion occurs. 
•  Add new keyword, *PARAMETER_TYPE, for use by LS-PrePost when combin-
ing  keyword  input  files.    The  appropriate  offset  is  applied  to  each  ID  value 
defined using *PARAMETER_TYPE, according to how that ID is used. 
•  Allow  use  of  load  curve  to  specify  damping  as  a  function  of  time  in  *DAMP-
ING_RELATIVE. 
•  Add a segment based (SOFT = 2) contact option to include the overlap area in the 
contact  stiffness  calculation.    This  is  good  for  improving the  friction  calculation 
and  possibly  for  implicit  convergence.    The  option  is  turned  on  by  setting 
FNLSCL > 0  and  DNLSCL = 0.    As  DNLSCL = 0,  the  contact  stiffness  is  not 
nonlinear.  This new option is also useful when used with another improvement 
that was made to the FS = 2 friction coefficient by table lookup option in segment 
based  contact.    When  the  above  mentioned  FNLSCL > 0,  option  is  used,  the 
FS = 2 option is now very accurate. 
•  Add  a  new  RCDC  damage  option,  *MAT_PLASTICITY_WITH_DAMAGE_OR-
THO_RCDC1980  which  is  consistent  with  the  WILKINS  paper.    It  uses  the 
principal values of stress deviators and a different expression for the A_d term. 
•  Add  a  TIETYP  option  to  *CONTACT_2D_AUTOMATIC.    By  default  the  tied 
contact  automatically  uses  constraint  equations  when  possible  for  2D  tied  con-
tact.  If a conflict is detected with other constraints, or to avoid 2-way constraints, 
penalty type ties are used when constraints are not possible.  The TIETYP option, 
when set to 1, causes all ties to use the penalty method.  This is useful if in spite 
of the code's best efforts to avoid problems, there is still a conflict in the model. 
•  Add a scale factor for scaling the frictional stiffness for contact.  The parameter is 
FRICSF on optional card E and it's only supported for segment based (SOFT = 2) 
contact.  This was motivated by a rubber vs.  road skidding problem where the 
friction  coefficent  had  static,  dynamic  and  decay  parameters  defined.    The 
growth of the frictional force was too slow so the static coulomb value could not 
be achieved.   By scaling the frictional stiffness higher, the  coulomb value could 
approach the static value. 
•  Add  keyword  *CONTACT_2D_AUTOMATIC_FORCE_TRANSDUCER.    Like 
the  3D  force  transducers,  it  does  no  contact  calculation  but  only  measures  the 
contact forces from other contact definitions.  When only a slave side is defined, 
the  contact  force  on  those  segments  is  measured.    Currently,  two  surface  force 
transducers are not available. 
•  Add options to *MAT_058: 
◦  Load  curves  for  rate  dependent  strain  values  (E11C,  E11T, …)  can  be  de-
fined on new optional card 9.
INTRODUCTION 
◦  Load curves for rate dependent strengths (XC, XT, …) and a rate averaging 
flag can be defined on new optional card 8. 
◦  Abscissa  values  in  above  curves  are  taken  to  be  natural  log  of  strain  rate 
when the first value is negative. 
◦  Add optional transverse shear damage to *MAT_058. 
•  Add  MAT_261  and  MAT_262  for  general  use.    *MAT_261  is  *MAT_LAMINA-
  *MAT_262  is  *MAT_LAMINATED_
TED_FRACTURE_DAIMLER_PINHO. 
FRACTURE_DAIMLER_CAMANHO. 
•  Add pentahedra cohesive solid element types (TYPE = 21 & 22).  Type = 21 is the 
pentahedra  version  of  Type = 19  and  Type = 22  is  the  pentahedra  version  of 
Type = 20.  Using ESORT.gt.0 in *CONTROL_SOLID will automatically sort out 
the pentahedra elements (19 to 21 and 20 to 22). 
•  Add  *DEFINE_DE_BY_PART  to  define  control  parameters  for  DES  by  part  ID, 
including  damping  coefficient,  friction  coefficient,  spring  constant,  etc.    If  de-
fined, it will overwrite the parameters in *CONTROL_DISCRETE_ELEMENT. 
•  Add new feature for *MAT_030 (*MAT_SHAPE_MEMORY) as optional 3rd card.  
Curves  or  tables  (strain  rate  dependency)  can  be  defined  to  describe  plastic 
loading and unloading behavior. 
•  New  feature  for  *ELEMENT_BEAM_PULLEY.    Beam  elements  BID1  and  BID2 
can now both be defined as “0” (zero).  In that case, adjacent beam elements are 
automatically  detected.    Therefore,  the  first  two  beam  elements  with  nodal 
distance < 1.0e-6 to the pulley node (PNID) will be chosen. 
•  Add  new  feature  to  *MAT_ADD_EROSION's  damage  model  GISSMO.    By 
default, damage is driven by equivalent plastic strain.  Now, users can optionally 
define another history variable as driving quantity by setting DMGTYP. 
•  Add volumetric plastic strain to *MAT_187 as history variable 6. 
•  Add internal energy calculation for *ELEMENT_BEAM_PULLEY. 
•  Add viscoplastic option to *MAT_157: new parameter VP on Card 5, Column 6. 
•  Add  new  keyword  *MAT_ADD_COHESIVE  which  is  intended  to  make  3D 
material models available for cohesive elements. 
•  Add new parameters to *MAT_CABLE_DISCRETE / *MAT_071.  MXEPS (Card 
2,  Column  4)  is  equal  the  maximum  strain  at  failure  and  MXFRC  (Card  2,  Col-
umn 5) is equal to the maximum force at failure 
•  Add  *MAT_124  as  potential  weld  partner  material  for  PROPRUL = 2/3  of  *DE-
FINE_CONNECTION_PROPERTIES. 
•  Add  new  material  *MAT_TOUGHENED_ADHESIVE_POLYMER  (TAPO)  or 
*MAT_252 for epoxy-based, toughened, ductile adhesives.
INTRODUCTION 
•  Add  new  option  to  *MAT_002_ANIS:  parameter  IHIS  on  Card  4,  Column  8.  
IHIS = 0: terms C11, C12, … from Cards 1, 2, and 3 are used.  IHIS = 1: terms C11, 
C12, … initialized by *INITIAL_STRESS_SOLID's extra history variables. 
•  Add new option to *MAT_102.  Instead of constant activation energy Q, one can 
define a load curve LCQ on Card 2, Column 7: 
◦  LCQ.GT.0: Q as function of plastic strain 
◦  LCQ.LT.0: Q as function of temperature 
•  Add  new  option  to  *MAT_071  (MAT_CABLE_DISCRETE_BEAM). 
  New 
parameter FRACL0 (Card 2, Column 3) is fraction of initial length that should be 
reached over time period of TRAMP.  That means the cable element length gets 
modified from L0 to FRACL0*L0 between t = 0 and t = TRAMP. 
•  Add internal energy calculation for SPR models *CONSTRAINED_INTERPOLA-
TION_SPOTWELD (SPR3) and *CONSTRAINED_SPR2.  Their contribution was 
missing in energy reports like glstat. 
•  Add  new  failure  model  OPT = 11  to  *MAT_SPOTWELD/*MAT_100  for  beam 
elements. 
•  Add  three  new  failure  criteria  for  shell  elements  to  *MAT_ADD_EROSION  on 
optional card 4, columns 6-8: 
◦  LCEPS12: load curve in-plane shear strain limit vs.  element size. 
◦  LCEPS13: load curve cross-thickness shear strain limit vs.  element size. 
◦  LCEPSMX: load curve in-plane major strain limit vs.  element size. 
•  Add  new  capability  to  *MAT_ADD_EROSION  damage  model  GISSMO.   Strain 
rate  scaling  curve  LCSRS  can  now  contain  natural  logarithm  values  of  strain 
rates  as  abscissa  values.    This  is  automatically  assumed  when  the  first  value  is 
negative. 
•  Add  new  parameter  NHMOD  to  *MAT_266.    The  constitutive  model  for  the 
isotropic part can now be chosen: 
◦  NHMOD = 0: original implementation (modified Neo-Hooke) 
◦  NHMOD = 1: standard Neo-Hookeon (as in umat45) 
•  New  keyword  *DEFINE_TABLE_MATRIX  is  an  alternative  way  of  defining  a 
table and the curves that the table references from a single unformatted text file, 
e.g., as saved from an Excel spreadsheet. 
•  Change long format so that all data fields are 20 columns and each line of input 
can hold up to 200 columns.  In this way, the number of input lines is the same 
for long format as for standard format. 
◦  8 variables per line in long format = 160 columns
INTRODUCTION 
◦  10 variables per line in long format = 200 columns 
•  Add  a  new  option  (SOFT = 6)  in  *CONTACT_FORMING_NODES_TO_SUR-
FACE for blank edge and guide pin contact. 
•  Add  user-defined  criteria  for  mesh  refinement  (or  coarsening)  in  *CONTROL_-
REFINE_…. 
•  Add new contact option that currently only works for MPP SINGLE_SURFACE 
contact with SOFT = 0 or 1.  If SRNDE (field 4 of optional card E) is a 1, then free 
edges  of  the  contact  definition  will  be  rounded  WITHOUT  extending  the  seg-
ments.    Rather  than  having  cylindrical  caps  on  the  ends  of  the  segments,  the 
“corners” of the squared off thickness are rounded over. 
•  Add geometric contact entity type -3 “finite cylinder”. 
•  Add  irate = 2  to  *CONTROL_IMPLICIT_DYNAMICS  to  turn  off  rate  effects  for 
both implicit and explicit. 
•  Add quadratic 8-node and 6-node shells (shell formulations 23 and 24). 
•  Add LOG_LOG_INTERPOLATION option for table defining strain rate effects in 
*MAT_083, *MAT_181, and *MAT_183. 
•  Add automatic generation of null shells for quadratic shell contact (*PART_DU-
PLICATE_NULL_OVERLAY). 
•  Add beam contact forces to rcforc output (*DATABASE_RCFORC).   
•  Add  SHL4_TO_SHL8  option  to  *ELEMENT_SHELL  to  automatically  convert  4-
node shells to 8-node quadratic shells. 
•  Add  3-node  beam  element  with  quadratic  interpolation  that  is  tailored  for  the 
piping  industry.    It  includes  12  degrees  of  freedom,  including  6  ovalization 
degrees of freedom, per node for a total of 36 DOF.  An internal pressure can be 
given that can stiffen and elongate the pipe. 
◦  ELFORM = 14 in *SECTION_BEAM. 
◦  *ELEMENT_BEAM_ELBOW.   
◦  NEIPB in *DATABASE_EXTENT_BINARY to direct output of elbow loop-
stresses to d3plot.  Otherwise, output goes to ASCII file elbwls.k. 
◦  Supported by a subset of material models including mats 3, 4, 6, 153, 195. 
•  Add discrete element option DE to *DATABASE_TRACER. 
◦  Includes variable RADIUS.  average result of all 
  RADIUS > 0: Reports the average result of all DE particles in a spher-
ical volume having radius = RADIUS and centered at the tracer. 
  RADIUS < 0: Reports result of the closest particle to the tracer.
INTRODUCTION 
◦   If a tracer node NID is given, then the tracer moves with this node.  The 
node must belong to a DES. 
•  Add  new  options  *PART_COMPOSITE_LONG  and  *ELEMENT_SHELL_COM-
POSITE_LONG.  In contrast to “COMPOSITE”, one integration point is defined 
per  card.    This  is  done  to  allow  for  more  informations,  e.g.    new  variable  “ply 
id”. 
•  Add  support  of  *MAT_ADD_EROSION  option  NUMFIP < 0  for  standard  (non-
GISSMO) failure criteria.  Only for shells. 
•  Add viscoplastic behavior to *MAT_157, i.e., parameter LCSS can now refer to a 
table with strain rate dependent yield curves. 
•  Add  singular  finite  element  with  midside  nodes  for  2D  plane  strain  fracture 
analysis (ELFORM = 55 in *SECTION_SHELL).  This is an 8-noded element and 
can  induce  a  singular  displacement  field  by  moving  mid-side  nodes  to  quarter 
locations. 
•  If HCONV < 0 in *AIRBAG_PARTICLE, |HCONV| is a curve of heat convection 
coefficient vs.  time. 
•  Add new option DECOMPOSITION for *AIRBAG_PARTICLE -- MPP only.This 
will  automatically  invoke  the  recommended  decomposition  commands,  *CON-
TROL_MPP_DECOMPOSITION_BAGREF    (if  applicable)  and  *CONTROL_-
MPP_DECOMPOSITION_ARRANGE_PARTS, for the bag. 
•  Add new blockage option for vents in *AIRBAG_PARTICLE: 
◦  blockage considered 
  .eq.0: no 
  .eq.1: yes 
  .eq.2: yes, exclude external vents 
  .eq.3: yes, exclude internal vents 
  .eq.4: yes, exclude all vents 
•  Add option in *CONTROL_CPM to consider CPM in the time step size calcula-
tion. 
•  When  using  *AIRBAG_PARTICLE  with  IAIR = 2,  user  should  keep  mole  / 
particle similar between inflator gas and initial air particles to ensure the correct 
elastic collision.  If different by more than 10%, code will issue warning message 
and provide the suggested initial air particle number. 
•  Enable  *DEFINE_CURVE_FUNCTION  for  *SECTION_POINT_SOURCE_MIX-
TURE and *SECTION_POINT_SOURCE. 
•  Make  *BOUNDARY_PRESCRIBED_MOTION_SET  compatible  with  *CON-
TROL_REFINE
INTRODUCTION 
•  Change  *BOUNDARY_ACOUSTIC_COUPLING_MISMATCH  to  rank  order 
opposing acoustic faces and structural segments by proximity, thereby accelerat-
ing  the  preprocessing  stage,  enhancing  reliability  and  allowing  some  liberaliza-
tion of the search parameters. 
•  Implement  hemispherical  geometry  for  particle  blast  (*DEFINE_PBLAST_-
GEOMETRY). 
•  Add explosive type for *PARTICLE_BLAST. 
•  For particle-based blast *PARTICLE_BLAST: 
◦  Include random distribution of initial air molecules 
◦  Modify  algorithm  to  account  for  the  non-thermally-equilibrated  state  of 
high velocity gas. 
•  Improve  particle  contact  method  for  particle-based  blast  loading  *PARTICLE_-
BLAST. 
•  *CONTACT now works for parts refined using *CONTROL_REFINE_SOLID or 
*CONTROL_REFINE_SHELL. 
•  Improve calculation of shell element contact segment thicknesses, particularly at 
material boundaries. 
•  MPP:  Add  output  to  rcforc  file  for  *CONTACT_AUTOMATIC_TIEBREAK  to 
record the # of nodes tied, and the total tied area. 
•  MPP: Add calculation of “contact gap” for master side of FORMING contact. 
•  MPP: Add support for table-based friction (FS = 2.0) to groupable contact. 
•  Implement  splitting-pinball  contact,  Belytschko  &  Yeh  (1992,  1993).    This  new 
contact  option  is  invoked  by  setting  SOFT = 2,  SBOPT = 3  and  DEPTH = 45.    A 
penetration  check  method  based  on  LS-PrePost  version  4.0  is  implemented  for 
the new bilinear-patch-based  contact, SOFT = 2, DEPTH = 45 & Q2TRI = 0.  The 
new method provides more accurate intersection information when Q2TRI = 0. 
•  Add support for birth time for *CONTACT_2D_AUTOMATIC_TIED. 
•  Improve the segment based single surface contact search for thick segment pairs 
that  are  too  close  together.    The  code  was  not  working  well  with  triangluar 
segments.    This  change  affects  models  with  shell  segments  that  have  thickness 
greater than about 2/3 of the segment length. 
•  Enable segment based quad splitting options to work when shell sets or segment 
sets  are  used  to  define  the  surface  that  will  be  split.    This  is  really  a  bug  fix 
because  there  was  no  check  to  prevent  this  and  the  result  was  writing  past  the 
allocated memory for segment connectivites. 
•  Allow  *CONSTRAINED_INTERPOLATION  to  use  node  set  to  define  the 
independent nodes.
INTRODUCTION 
•  Add a length unit to the tolerance used for the checking of noncoincident nodes 
in  *CONSTRAINED_JOINTs  excluding  spherical  joints.    The  old  tolerance  was 
1.e-3.  The new tolerance is 1.e-4 times the distance between nodes 1 and 3.  The 
error  messages  were  changed  to  warnings  since  this  change  might  otherwise 
cause existing models to stop running. 
•  Add  d3hsp  output 
for  *CONSTRAINED_INTERPOLATION_SPOTWELD 
(SPR3)  and  *CONSTRAINED_SPR2.    Can  be  deactivated  by  setting  NPOPT = 1 
on *CONTROL_OUTPUT. 
•  Support  NFAIL1  and  NFAIL4  of  *CONTROL_SHELL  in  coupled  thermal-
mechanical analysis, i.e.  erode distorted elements instead of error termination. 
•  PTSCL on *CONTROL_CONTACT can be used to scale contact force exerted on 
shell formulations 25, 26, 27 as well as shell formulations 2, 16 (IDOF = 3). 
•  Use SEGANG in *CONTROL_REMESHING to define positive critical angle (unit 
is radian) to preserve feature lines in 3D tetrahedral remeshing (ADPOPT = 2 in 
*PART). 
•  For  3D  solid  adaptive  remeshing  including  ADPOPT = 2  and  ADPOPT = 3 
(*PART), the old mesh will be used automatically if the remesher fails generating 
a new mesh. 
•  Add option INTPERR on *CONTROL_SHELL (Optional Card 3, Column 8).  By 
default, warning messages INI+143/144/145 are written in case of non-matching 
number  of  integration  points  between  *INITIAL_STRESS_SHELL  and  *SEC-
TION_SHELL.  Now with INTPERR = 1, LS-DYNA can terminate with an error. 
•  Add  variable  D3TRACE  on  *CONTROL_ADAPTIVE:  The  user  can  now  force  a 
plot  state  to  d3plot  just  before  and  just  after  an  adaptive  step.    This  option  is 
necessary for tracing particles across adaptive steps using LS-PrePost. 
•  By  putting  MINFO = 1  on  *CONTROL_OUTPUT,  penetration  info  is  written  to 
message files for mortar contact., see also *CONTACT_….  Good for debugging 
implicit models, not available for explicit. 
•  Change the default scale factor for binary file sizes back to 70.  This value can be 
changed using “x=” on the execution line.  In version R7.0, the default value of x 
is  4096,  and  that  sometimes  leads  to  difficulty  in  postprocessing  owing  to  the 
large size of the d3plot file(s). 
•  Enable *CONTROL_OUTPUT flag, EOCS, which wasn't having any effect on the 
shells output to elout file. 
•  *DATABASE_FSI_SENSOR: Create sensors at solid faces in 3D and at shell sides 
in 2D. 
•  *DATABASE_PROFILE:  Implement  the  option  DIR = 4  to  plot  data  with 
curvilinear distributions and the flag UPDLOC to update the profile positions. 
•  In *CONTROL_SHELL, add options for deletion of shells based on:
INTRODUCTION 
◦  diagonal stretch ratio (STRETCH) 
◦  w-mode amplitude in degrees (W-MODE) 
•  New  element  formulation  ELFORM = 45  in  *SECTION_SOLID:  Tied  Meshfree-
enriched FEM (MEFEM).  This element is based on the 4-noded MEFEM element 
(ELFORM = 43,  *SECTION_SOLID).    Combined  with  *CONSTRAINED_TIED_-
NODES_FAILURE,  *SET_NODE_LIST  and  cohesive  model,  this  element  can  be 
used  to  model  dynamic  multiple-crack  propagation  along  the  element  bounda-
ries. 
•  New  high  order  tetrahedron  CPE3D10  based  on  Cosserat  Point  theory  can  be 
invoked  by  specifying  element  formulation  ELFORM = 16  and  combining  this 
with  hourglass  formulation  IHQ = 10.    See  *SECTION_SOLID  and  *HOUR-
GLASS. 
•  Add database D3ACS for collocation acoustic BEM (*FREQUENCY_DOMAIN_-
ACOUSTIC_BEM) to show the surface pressure and normal velocities. 
•  Implement  biased  spacing  for  output  frequencies  for  random  vibration  (*FRE-
QUENCY_DOMAIN_RANDOM_VIBRATION). 
•  Add  frequency  domain  nodal  or  element  velocity  output  for  acoustic  BEM 
(*FREQUENCY_DOMAIN_ACOUSTIC_BEM). 
•  Implement  boundary  acoustic  mapping  to  acoustic  BEM  in  MPP  (*BOUND-
ARY_ACOUSTIC_MAPPING).  This is enabled only for segment sets  at present. 
•  Implement  panel  contribution  analysis  capability  to  Rayleigh  method  (*FRE-
QUENCY_DOMAIN_ACOUSTIC_BEM_PANEL_CONTRIBUTION). 
•  Implement a scheme to map velocity boundary condition from dense BEM mesh 
to  coarse  mesh  to  speed  up  the  computation  (*FREQUENCY_DOMAIN_-
ACOUSTIC_BEM). 
•  Add  user  node  ID  for  acoustic  field  points  in  D3ATV  (*FREQUENCY_DO-
MAIN_ACOUSTIC_BEM).    Now  D3ATV  is  given  for  multiple  field  points,  and 
multiple frequencies. 
•  Add  database  D3ATV  for  acoustic  transfer  vector  binary  plot  (*FREQUENCY_-
*DATABASE_FREQUENCY_BINARY_-
DOMAIN_ACOUSTIC_BEM_ATV, 
D3ATV). 
•  Implement  acoustic  panel  contribution  analysis  to  collocation  BEM  and  dual 
collocation BEM (*FREQUENCY_DOMAIN_ACOUSTIC_BEM). 
•  Enable  *FREQUENCY_DOMAIN_MODE  in  response  spectrum  analysis  (*FRE-
QUENCY_DOMAIN_RESPONSE_SPECTRUM). 
•  Implement  an  option  to  read  in  user-specified  nodal  velocity  history  data  for 
running BEM acoustics (*FREQUENCY_DOMAIN_ACOUSTIC_BEM).
INTRODUCTION 
•  Extend  Kirchhoff  acoustic  method 
to  MPP 
(*FREQUENCY_DOMAIN_-
ACOUSTIC_BEM). 
•  Extend  response  spectrum  analysis  to  multiple  load  spectra  cases  (*FREQUEN-
CY_DOMAIN_RESPONSE_SPECTRUM). 
•  Add BAGVENTPOP for *SENSOR_CONTROL.  This allows user more flexibilty 
controlling  the  pop-up  of  the  venting  hole  of  *AIRBAG_HYBRID  and 
*AIRBAG_WANG_NEFSKE 
•  Add  command  *SENSOR_DEFINE_FUNCTION.    Up  to  15  *DEFINE_SENSORs 
can be referenced in defining a mathematical operation. 
•  LAYER  of  *SENSOR_DEFINE_ELEMENT  can  now  be  an  integer  “I”  represent-
ing  the  Ith  integration  point  at  which  the  stress/strain  of  the  shell  or tshell  ele-
ment will be monitored. 
•  Add control of *LOAD_MOVING_PRESSURE by using *SENSOR_CONTROL. 
•  Add thick shells to the ETYPE option list of *SENSOR_DEFINE_ELEMENT. 
•  Add  *CONTROL_MPP_MATERIAL_MODEL_DRIVER  in  order  to  enable  the 
Material Model Driver for MPP (1 core). 
•  Add  table  input  of  thermal  expansion  coefficient  for  *MAT_270.    Supports 
temperature-dependent curves arranged according to maximum temperature. 
•  Add table input of heat capacity for *MAT_T07.  Supports temperature depend-
ent curves arranged according to maximum temperature. 
•  Add two more kinematic hardening terms for *MAT_DAMAGE_3/MAT_153, c2 
& gamma2. 
•  Add materials *MAT_CONCRETE_DAMAGE_REL3/*MAT_072R3 and *MAT_-
CSCM_CONCRETE/*MAT_159 to Interactive Material Model Driver. 
•  Enable  *MAT_JOHNSON_COOK/*MAT_015  for  shell  elements  to  work  with 
coupled structural / thermal analysis. 
•  Allow *MAT_SOIL_AND_FOAM/*MAT_005 to use positive or negative abscissa 
values forload curve input of volumetric strains. 
•  Add *MAT_ACOUSTIC elform = 8 support for pyramid element case using 5-pt 
integration. 
•  Add support to *MAT_219 (*MAT_CODAM2) for negative AOPT values which 
point to coordinate system ID's. 
•  Modify  *MAT_224  so  it  uses  the  temperatures  from  the  thermal  solution  for  a 
coupled thermal-mechanical problem. 
•  Add  alternative  solution  method  (Brent)  for  *MAT_015  and  *MAT_157  in  case 
standard iteration fails to converge.
INTRODUCTION 
•  Add  shell  element  IDs  as  additional  output  to  messag  file  for  *MAT_036's 
warning “plasticity algorithm did not converge”. 
•  For  *MAT_USER_DEFINED_MATERIAL_MODELS,  the  subroutines  crvval  and 
tabval can be called with negative curve / table id which will extract values from 
the  user  input  version  of  the  curve  or  table  instead  of  the  internally  converted 
“100-point” curve / table. 
•  In  the  damage  initiation  and  evolution  criteria  of  *MAT_ADD_EROSION 
(invoked by IDAM < 0), add the option Q1 < 0 for DETYP = 0.  Here, |Q1| is the 
table ID defining the ufp (plastic displacement at failure) as a function of triaxial-
ity and damage value, i.e., ufp = ufp(eta, D), as opposed to being constant which 
is the default. 
•  In  *MAT_RHT,  ONEMPA = -6  generates  parameters  in  g,  cm,  and  𝜇S  and 
ONEMPA = -7 generates parameters in g, mm, and mS 
•  In  *MAT_SIMPLIFIED_RUBBER/FOAM,  STOL > 0  invokes  a  stability  analysis 
and  warning  messages  are  issued  if  an  unstable  stretch  point  is  found  within  a 
logarithmic strain level of 100%. 
•  Implement  *DATABASE_ALE  to  write  time  history  data  (volume  fractions, 
stresses, …) for a set of ALE elements.  Not to be confused with *DATABASE_-
ALE_MAT. 
•  Implement *DELETE_PART in small restarts for ALE2D parts. 
•  Add  conversion  of  frictional  contact  energy  into  heat  when  doing  a  coupled 
thermal-mechanical  problem  for  SPH  (variable  FRCENG  in  *CONTROL_CON-
TACT).  This option applys to all 3D contact types supported by SPH particles. 
•  For  keyword  *DEFINE_ADAPTIVE_SOLID_TO_SPH,  add  support  of  explicit 
SPH thermal solver for the newly generated SPH particles which were converted 
from solid elements.   The temperatures of those newly generated SPH particles 
are mapped from corresponding solid elements. 
•  Implement  DE  to  surface  tied  contact  *DEFINE_DE_TO_SURFACE_TIED.    The 
implementation includes bending and torsion. 
•  Implement  keyword  *DEFINE_DE_HBOND  to  define  heterogeneous  bond  for 
discrete  element  spheres  (DES).    DES  (*ELEMENT_DISCRETE_SPHERE)  with 
different material models can be bonded. 
•  Implement keyword *INTERFACE_DE_BOND to define multiple failure models 
for  various  bonds  within  one  part  or  between  different  parts  through  the  key-
word *DEFINE_DE_HBOND. 
•  Implement  *DEFINE_DE_TO_BEAM_COUPLING  for  coupling  of  discrete 
element spheres to beam elements.
INTRODUCTION 
•  Add variable MAXGAP in *DEFINE_DE_BOND to give user control of distance 
used in judging whether to bond two DES together or not, based on their initial 
separation. 
•  Add  IAT = -3  in  *CONTROL_REMESHING_EFG,  which  uses  FEM  remapping 
scheme in EFG adaptivity.  Compared to IAT = -2, -1, 1, 2, IAT = -3 is faster and 
more robust but less accurate. 
•  Add  control  flag  MM  in  *CONTROL_REMESHING_EFG  to  turn  on/off 
monotonic  mesh  resizing  for  EFG  3D  general  remeshing  (ADPOPT = 2  in 
*PART). 
•  *CONTROL_IMPLICIT_BUCKLING - Extend Implicit Buckling Feature to allow 
for  Implicit  problems  using  Inertia  Relief.    This  involves  adding  the  Power 
Method  as  a  solution  technology  for  buckling  eigenvalue  problems.    Using  the 
power method as an option for buckling problems that are not using inertia relief 
has been added as well. 
•  Extend  Implicit  Buckling  to  allow  for  Intermittent  extraction  by  using  negative 
values  of  NMODE  on  *CONTROL_IMPLICIT_BUCKLING  similar  to  using 
negative values of NEIG on *CONTROL_IMPLICIT_EIGENVALUE. 
•  Extend implicit-explicit switching specified on *CONTROL_DYNAMIC_RELAX-
ATION to allow explicit simulation for the dynamic relaxation phase and implic-
it for the transient phase. 
•  New  implementation  for  extracting  resultant  forces  due  to  joints  for  implicit 
mechanics. 
•  New implementation of extracting resultant forces due to prescribed motion for 
implicit mechanics. 
•  Add support for IGAP > 2 in implicit, segment based (SOFT = 2) contact. 
•  Add  constraint-based,  thermal  nodal  coupling  for  *CONSTRAINED_LA-
GRANGE_IN_SOLID.  HMIN < 0 turns it on. 
•  Add FRCENG = 2 on CONTROL_CONTACT keyword. 
◦  if FRCENG = 1, convert contact frictional energy to heat. 
◦  if FRCENG = 2, do not convert contact frictional energy to heat. 
•  Add effect of thermal time scaling (TSF in *CONTROL_THERMAL_SOLVER) to 
2D contact. 
•  Add  new  pfile  decomposition  region  option:  partsets.    Takes  a  list  of  part  sets 
(*SET_PART)  from  the  keyword  input  and  uses  them  to  define  a  region,  e.g., 
region { partsets 102 215 sy 1000 } This example would take partsets, scale y by 
1000, and decompose them and distribute them to all processors. 
•  Reduce MPP memory usage on clusters. 
•  Add MPP support for *ELEMENT_SOURCE_SINK.
INTRODUCTION 
•  Add new pfile options: 
◦  decomp { d2r_as_rigid } 
◦  decomp { d2ra_as_rigid } 
which  cause  materials  appearing  in  “*DEFORMABLE_TO_RIGID”  and  “*DE-
FORMABLE_TO_RIGID_AUTOMATIC” to have their computational costs set as 
if they were rigid materials during the decomposition. 
•  Add  option  ISRCOUT  to  *INCLUDE_STAMPED_PART  to  dump  out  the 
transformed source/stamp mesh. 
•  *CONTROL_FORMING_OUTPUT: Allow NTIMES to be zero; support birth and 
death time; support scale factor in curve definition. 
•  Add a new option (INTFOR) to *CONTROL_FORMING_OUTPUT to control the 
output frequency of the INTFOR database. 
•  Add  new  features  (instant  and  progressive  lancing)  in  *ELEMENT_LANCING 
for sheet metal lancing simulation. 
•  Add a new keyword: *CONTROL_FORMING_INITIAL_THICKNESS. 
•  Add  a  new  option  for  springback  compensation:  *INCLUDE_COMPENSA-
TION_ORIGINAL_TOOLS. 
•  Add 
a  new 
keyword: 
*INTERFACE_COMPENSATION_NEW_PART_-
CHANGE. 
•  Add  a  new  keyword  (*DEFINE_CURVE_BOX_ADAPTIVITY)  to  provide  better 
control of mesh refinement along two sides of the curve. 
•  Isogeometric analysis: contact is available in MPP. 
•  Normalize  tangent  vectors  for  local  coordinate  system  for  the  rotation  free 
isogeometric shells. 
•  Add  support  for  dumping  shell  internal  energy  density  for  isogeometric  shells 
(*ELEMENT_SHELL_NURBS_PATCH) via interpolation shells. 
•  Add support for dumping of strain tensor (STRFLG.eq.1) for isogeometric shells 
(*ELEMENT_SHELL_NURBS_PATCH) via interpolation shells. 
•  Add H-field, magnetization and relative permeability to d3plot output. 
•  *ICFD_INITIAL: Add a reference pressure (pressurization pressure) for when no 
pressure is imposed on the boundaries. 
•  Add the initialization of all nodes at once by setting PID = 0. 
•  Add  the  non-inertial  reference  frame  implementation  defined  by  the  keyword 
*ICFD_DEFINE_NONINERTIAL. 
•  Add several new  state variables to LSO.  Please refer to the LSO manual to see 
how to print out the list of supported variables.
INTRODUCTION 
•  Add support for FSI with thick shells. 
•  2D  shells  are  now  supported  for  FSI  in  MPP.    In  the  past  only  beams  could  be 
used in MPP and beams and shells could be used in SMP. 
•  The keyword ICFD_CONTROL_FSI has a new field to control the sensitivity of 
the algorithm to find the solid boundaries used in FSI calculations. 
•  The 2D mesh now generates semi-structured meshes near the boundaries. 
•  Add heat flux boundary condition using ICFD_BOUNDARY_FLUX_TEMP. 
•  Add divergence-free and Space Correlated Synthetic Turbulence Inlet Boundary 
Condition  for  LES  (Smirnov  et  al.)  using  *ICFD_BOUNDARY_PRESCRIBED_-
VEL. 
•  *ICFD_BOUNDARY_PRESCRIBED_VEL:  Add  inflow  velocities  using  the  wall 
normal and a velocity magnitude using the 3rd field VAD. 
•  Add the activation of synthetic turbulence using the 3rd field VAD. 
•  Add  the  option  to  control  the  re-meshing  frequency  in  both  keywords:  see 
*ICFD_CONTROL_ADAPT_SIZE and *ICFD_CONTROL_ADAPT. 
•  *ICFD_CONTROL_TURB_SYNTHESIS:  control  parameters  for  the  synthetic 
turbulence inflow. 
•  *ICFD_BOUNDARY_PRESCRIBED_MOVEMESH:  Allows  the  mesh  to  slide  on 
the boundaries following the cartesian axis. 
•  Add a PART_SET option for *CESE_BOUNDARY_…_PART cards. 
•  Bring  in  more  2D  mesh  support,  both  from  the  PFEM  mesher  and  a  user  input 
2D mesh (via *ELEMENT_SOLID with 0 for the last 4 of 8 nodes). 
•  Enable the 2D ball-vertex mesh motion solver for the 2D CESE solver. 
•  Add new input cards: 
◦  *CESE_BOUNDARY_CYCLIC_SET 
◦  *CESE_BOUNDARY_CYCLIC_PART 
•  Add code for 2D CESE sliding boundary conditions. 
•  Add support in CESE FSI for 2D shells in MPP. 
•  Add support for CESE FSI with thick shells. 
•  Add  2D  &  2D-axisymmetric  cases  in  the  CESE-FSI  solver  (including  both 
immersed boundary method & moving mesh method) . 
•  Add  the  CSP  reduced  chemistry  model  with  0D,  2D,  and  3D  combustion.    The 
2D and 3D combustion cases couple with the CESE compressible flow solver. 
•  Add the G-scheme reduced chemistry model only for 0D combustion. 
•  Add two different reduced chemistry models.
INTRODUCTION 
◦  The  Computational  Singular  Perturbation  (CSP)  reduced  model  is  imple-
mented with existing compressible CESE solver.  The CSP is now working 
on  0-dimensional  onstant  volume  and pressure  combustion,  2-D,  and  3-D 
combustion problems. 
◦  The  new  reduced  chemistry  model,  G-scheme,  is  implemented,  but  cur-
rently works only 0-dimensional problems such as constant combustors. 
•  Jobid  can  now  be  changed  in  a  restart  by  including  “jobid=“  on  the  restart 
execution line.  Previously, the jobid stored in d3dump could not be overwritten. 
•  Part  labels  (PID)  can  be  up  to  8  characters  in  standard  format;  20  characters  in 
long format. 
•  Labels for sections (SID), materials (MID), equations of state (EOSID), hourglass 
IDs (HGID), and thermal materials (TMID) can be up to 10 characters in standard 
format; 20 characters in long format. 
•  Create  bg_switch  and  kill_by_pid  for  SMP.    Both  files  will  be  removed  at  the 
termination of the run. 
•  Increase the overall length of command line to 1000 characters and length of each 
command line option to 50 characters. 
•  Increase  MPP  search  distance  for  tied  contacts  to  include  slave  and  master 
thicknesses. 
•  For *CONTACT_AUTOMATIC_…_MORTAR, the mortar contact now supports 
contact with the lateral surface of beam elements. 
•  On  *CONTACT_..._MORTAR,  IGAP.GT.1  stiffens  the  mortar  contact  for  large 
penetrations.  The mortar contact has a maximum penetration depth DMAX that 
depends  on  geometry  and  input  parameters;  if  penetration  is  larger  than  this 
value  the  contact  is  released.    To  prevent  this  release,  which  is  unwanted,  the 
user may put IGAP.GT.1 which stiffens the behavior for penetrations larger than 
0.5*DMAX  without  changing  the  behavior  for  small  penetrations.    This  should 
hopefully not be as detrimental to convergence as increasing the overall contact 
stiffness. 
•  For  initialization  by  prescribed  geometry  in  dynamic  relaxation  (IDRFLG = 2, 
*CONTROL_DYNAMIC_RELAXATION),  add  an  option  where  displacements 
are not imposed linearly but rather according to a polar coordinate system.  This 
option was added to accommodate large rotations. 
•  The  flag  RBSMS  on  *CONTROL_RIGID  is  now  active  for  regular  and  selective 
mass scaling to consistently treat interfaces between rigid and deformable bodies 
•  Remove  static  linking  for  l2a  as  many  systems  do  not  have  the  required  static 
libraries. 
•  Add  IELOUT  in  *CONTROL_REFINE  to  handle  how  child  element  data  is 
handled  in  elout  (*DATABASE_HISTORY_SOLID  and  *DATABASE_HISTO-
INTRODUCTION 
RY_SHELL).  Child element data are stored if IELOUT = 1 or if refinement is set 
to occur only during initialization. 
•  Include  eroded  hourglass  energy  in  hourglass  energy  in  glstat  file  to  be  con-
sistent  with  KE  &  IE  calculations  so  that  the  total  energy = kinetic  energy  + 
internal energy + hourglass energy + rigidwall energy. 
•  Remove *DATABASE_BINARY_XTFILE since it is obsolete. 
•  When  using  *PART_AVERAGED  for  truss  elements  (beam  formulation  3), 
calculate the time step based on the total length of the combined macro-element 
instead of the individual lengths of each element. 
•  Enable  writing  of  midside  nodes  to  d3plot  or  6-  and  8-node  quadratic  shell 
elements. 
•  Write complete history variables to dynain file for 2D solids using *MAT_NULL 
and equation-of-state. 
•  Shell  formulations  25,  26,  and  27  are  now  fully  supported  in  writing  to  dynain 
file (*INTERFACE_SPRINGBACK_LSDYNA). 
•  Shell formulations 23 (quad) and 24 (triangle) can now be mixed in a single part.  
When  ESORT = 1  in  *CONTROL_SHELL,  triangular  shells  assigned  by  *SEC-
TION_SHELL to be type 23 will automatically be changed to type 24. 
•  Enable hyperelastic materials (those that use Green's strain) to be used with thick 
shell form 5.  Previously, use of these materials (2, 7, 21, 23, 27, 30, 31, 38, 40, 112, 
128, 168, and 189) with thick shell 5 has been an input error. 
•  Update  acoustic  BEM  to  allow  using  *DEFINE_CURVE  to  define  the  output 
frequencies (*FREQUENCY_DOMAIN_ACOUSTIC_BEM). 
•  When  using  *CONTROL_SPOTWELD_BEAM,  convert  *DATABASE_HISTO-
RY_BEAM  to  *DATABASE_CROSS_SECTION  and  *INITIAL_AXIAL_FORCE_-
BEAM to *INITIAL_STRESS_CROSS_SECTION for the spotweld beams that are 
converted to hex spotwelds. 
•  Improve output of *INITIAL_STRESS_BEAM data to dynain via *INTERFACE_-
SPRINGBACK_LSDYNA.    Now,  large  format  can  be  chosen,  history  variables 
are written, and local axes vectors are included. 
•  Update *MAT_214 (*MAT_DRY_FABRIC) to allow fibers to rotate independent-
ly. 
•  Enable regularization curve LCREGD of *MAT_ADD_EROSION to be used with 
FLD  criterion,  i.e.    load  curve  LCFLD.    Ordinate  values  (major  strain)  will  be 
scaled with the regularization factor. 
•  Modify *MAT_ADD_EROSION parameter EPSTHIN: 
◦  EPSTHIN > 0: individual thinning for each IP from z-strain (as before). 
◦  EPSTHIN < 0: averaged thinning strain from element thickness (new).
INTRODUCTION 
•  Enable regularization curve LCREGD of *MAT_ADD_EROSION to be used with 
standard (non-GISSMO) failure criteria.  Users can now define a failure criterion 
plus IDAM = 0 plus LCREGD = scaling factor vs.  element size to get a regular-
ized failure criterion. 
•  *MAT_ADD_EROSION:  equivalent  von  Mises  stress  SIGVM  can  now  be  a 
function of strain rate by specifying a negative load curve ID. 
•  *SECTION_ALE1D  and  *SECTION_ALE2D  now  work  on  multiple  processors 
(SMP and MPP). 
•  *CONSTRAINED_LAGRANGE_IN_SOLD  ctype  4/5  now  converts  friction 
energy to heat.  Note it only works for ALE elform 12. 
Capabilities added  September 2013 – January 2015 to create LS-DYNA R8.0:  
See release notes (published separately) for further details. 
•  Add RDT option for *AIRBAG_SHELL_REFERENCE_GEOMETRY.  
•  LCIDM  and  LCIDT  of  *AIRBAG_HYDRID  can  now  be  defined  through  *DE-
FINE_CURVE_FUNCTION. 
•  New  variable  RGBRTH  in  *MAT_FABRIC  to  input  part-dependent  activation 
time for airbag reference geometry. 
•  Negative  PID  of  *AIRBAG_INTERACTION  considers  the  blockage  of  partition 
area due to contact. 
•  Enhancements to *AIRBAG_PARTICLE: 
◦  New blockage (IBLOCK) option for vents. 
◦  External work done by inflator gas to the structure is reported to glstat. 
◦  Enhance segment orientation checking of CPM bag and chambers. 
◦  Allow user to excluded some parts surface for initial air particles. 
◦  Support compressing seal vent which acts like flap vent. 
◦  Support Anagonye and Wang porosity equation through *MAT_FABRIC. 
◦  Add keyword option _MOLEFRACTION. 
•  Add_ID  keyword  option 
*AIRBAG_REFERENCE_GEOMETRY  and 
*AIRBAG_SHELL_REFERENCE  which  includes  optional  input  of  variables  for 
scaling the reference geometry. 
to 
•  Enable  *DEFINE_CURVE_FUNCTION  for  *AIRBAG_SIMPLE_AIRBAG_MOD-
EL. 
•  Calculate  heat  convection  (HCONV)  between  environment  and  airbag  in 
consistent fashion when TSW is used to switch from a particle airbag to a control 
volume.
INTRODUCTION 
•  For  *AIRBAG_PARTICLE,  add  ENH_V = 2  option  for  vent  hole  such  that  two-
way flow can occur, i.e., flow with or against the pressure gradient. 
•  *BOUNDARY_ALE_MAPPING:  add  the  following  mappings:  1D  to  2D,  2D  to 
2D, 3D to 3D. 
•  *SET_POROUS_ALE:  new  keyword  to  define  the  properties  of  an  ALE  porous 
media by an element  set.  The porous forces are computed by *LOAD_BODY_-
POROUS. 
•  *ALE_FSI_SWITCH_MMG: applies also now to 2D. 
•  *ALE_SWITCH_MMG:  new  keyword  to  switch  multi-material  groups  based  on 
criteria defined by the user with *DEFINE_FUNCTION. 
•  *CONTROL_ALE: Allow PREF (reference pressure) to be defined by materials. 
•  Implement *ALE_COUPLING_NODAL_DRAG to model the drag force coupling 
between discrete element spheres or SPH particles and ALE fluids. 
•  Implement  *ALE_COUPLING_RIGID_BODY  as  an  efficient  alternative  for 
constraint type coupling between ALE fluids and a Lagrangian rigid body. 
•  Error  terminate  if  *BOUNDARY_SPC_NODE_BIRTH_DEATH  is  applied  to  a 
node that belongs to a rigid body. 
•  Modify  *BOUNDARY_PRESCRIBED_ORIENTATION_VECTOR  to  accommo-
date bodies which undergo no changes in orientation. 
•  Add a new keyword *BOUNDARY_SPC_SYMMETRY_PLANE. 
•  Solid part or solid part set is now allowed for *PARTICLE_BLAST. 
•  Add ambient pressure boundary condition flag BC_P for *PARTICLE_BLAST. 
•  New  command  *DEFINE_PBLAST_GEOMETRY  allows  the  high  explosive 
domain for*PARTICLE_BLAST to be defined by various geometric shapes. 
•  Allow multiple *PARTICLE_BLAST definitions. 
•  Add *DATABASE_PBSTAT to output particle blast statistics. 
•  Output  the  initial  volume  and  initial  mass  of  HE  particles  and  air  particles  for 
*PARTICLE_BLAST to d3hsp.  
•  Add  the  command  *CESE_BOUNDARY_BLAST_LOAD  to  allow  a  blast 
described  by  the  *LOAD_BLAST_ENHANCED  command  to  be  used  as  a 
boundary condition in CESE.  
•  Modify  the  FSI  interface  reflective  boundary  condition  pressure  treatment  in 
some calculations for the moving mesh and immersed boundary solvers. 
•  Change  the  CESE  derivatives  calculation  method  to  use  the  current  values  of 
flow variables.
INTRODUCTION 
•  Add two new MAT commands for CESE solver, *CESE_MAT_000 and *CESE_-
MAT_002.  
•  Add a non-inertial reference frame solver for fluid and  FSI problems using the 
moving-mesh method.  
•  For  the  moving  mesh  CESE  solver,  replace  the  all-to-all  communication  for 
conjugate heat and FSI quantities with a sparse communication mechanism. 
•  Add  structural  element  erosion  capability  to  the  immersed  boundary  method 
CESE FSI solver (serial capability only). 
•  Add 2D cyclic boundary conditions capability. 
•  Add a NaN detection capability for the CESE solver. 
•  Switch all CESE boundary conditions that use a mesh surface part to define the 
boundary  to  use  the  character  string  "MSURF"  instead  of  "PART"  in  the  option 
portion of the keyword name. 
•  Add missing temperature interpolation in time for imposing solid temperatures 
as a boundary condition in the CESE solver. 
•  Optimize the IDW-based mesh motion for the CESE moving mesh solver. 
•  Treat the input mesh as 3D by default for the CESE solver. 
•  All  of  the  chemistry  features  mentioned  below  are  coupled  only  to  the  CESE 
compressible flow solver when 2D or 3D calculations are involved. 
•  Chemical source Jacobians have been added. 
•  Introduce  *CHEMISTRY_CONTROL_PYROTECHNIC  and  *CHEMISTRY_PRO-
PELLANT_PROPERTIES for airbag applications.  In conjuction with these com-
mands, basic airbag inflator models are implemented. 
•  The  pyrotechnic  inflator  model  using  NaN3/Fe2O3  propellant  is  newly 
implemented.  To connect with the existing ALE airbag solver, two load curves, 
mass  flow  rate  and  temperature,  are  saved  in  "inflator_outfile"  as  a  function  of 
time.  This model computes three sub-regions: combustion chamber, gas plenum, 
and discharge tank.  Each region can be initialized with different *CHEMISTRY_-
COMPOSITION  models,  which  means  that  user  can  compute  Propellant+Gas 
hybrid mode. 
•  The  following  0-dimensional  combustion  problems  have  been  improved: 
constant volume, constant pressure, and CSP. 
•  For iso-combustion.  temperature and species mass fractions as a function of time 
are displayed on screen and saved in "isocom.csv" to plot with LS-PrePost. 
•  Another chemical ODE integration method has been implemented. 
•  The output file of the pyrotechnic inflator is updated so that this file can be read 
from ALE solver for an airbag simulation.
INTRODUCTION 
•  2-D  and  3-D  TNT  gaseous  blast  explosives,  categorized  as  TBX  (thermobaric 
explosives), are implemented for the Euler equation systems (CESE-only).  Also, 
3-D TNT blast + aluminum combustion for serial problems is now implemented. 
•  Implement a mix modeling method for use with CESE solvers. 
•  Modify  *CHEMISTRY-related  keyword  commands  to  allow  multiple  chemistry 
models in the same problem. 
•  Add  command  *CHEMISTRY_MODEL  which  identifies  the  files  that  define  a 
Chemkin chemistry model. 
•  Modify  the  following  commands  such  that  the  files  related  to  the  chemistry 
model have been removed.  These commands are only used to select the type of 
chemistry solver: 
◦  *CHEMISTRY_CONTROL_CSP 
◦  *CHEMISTRY_CONTROL_FULL 
◦  *CHEMISTRY_CONTROL_1D 
•  Modify  *CHEMISTRY_DET_INITIATION  where  the  files  related  to  the  chemis-
try  model  have  been  removed,  and  the  Model  ID  used  is  inferred  through  a 
reference to a chemistry composition ID. 
•  Modify  *CHEMISTRY_COMPOSITION  and  *CESE_CHEMISTRY_D3PLOT  to 
add model ID. 
•  Add  *CONTACT_TIED_SHELL_EDGE_TO_SOLID  for  transferring  moments 
from shells into solids. 
•  Add frictional energy calculation for beams in *CONTACT_AUTOMATIC_GEN-
ERAL. 
•  Enhance  ERODING  contacts  for  MPP.    The  new  algorithm  uses  a  completely 
different approach to determining the contact surface.  The old algorithm started 
from  scratch  when  identifying  the  exterior  of  the  parts  in  contact.    The  new 
algorithm  is  smarter  about  knowing  what  has  been  exposed  based  on  what  is 
eroded, and is faster. 
•  Force EROSOP = 1 for all ERODING type contacts, with a warning to the user if 
they had input it as 0. 
•  Add  error  check  in  case  of  a  contact  definition  with  an  empty  node  set  being 
given for the slave side. 
•  Modify output of ncforc (*DATABASE_NCFORC) in order to support output in 
a local coordinate system. 
•  For ERODING contacts, reduce memory allocated for segments so each interior 
segment is only allocated once. 
•  Add  keyword  *DEFINE_CONTACT_EXCLUSION  (MPP  only)  to  allow  for 
nodes tied in some contacts to be ignored in certain other contacts.
INTRODUCTION 
•  Rewrite  meshing  of  *CONTACT_ENTITY  to  use  dynamic  memory,  which 
removes the previous limit of 100 meshed contact entities.  There is now no limit. 
•  Remove  undocumented  release  condition  for  MPP’s  *CONTACT_AUTOMAT-
IC_TIEBREAK, options 5 and greater. 
•  Add new experimental "square edge" option to select SOFT = 0,1 contacts.  This 
new option applies only to AUTOMATIC_SINGLE_SURFACE and the segment-
to-segment  treatment  of  AUTOMATIC_GENERAL,  and  is  invoked  by  setting 
SRNDE = 2 on *CONTACT's Optional Card E. This new option does not apply to 
SOFT = 2;  SOFT = 2  square  edge  option  is  set  using  SHLEDG  in  *CONTROL_-
CONTACT. 
•  BT  and  DT  in  *CONTACT  can  be  set  to  define  more  than  one  pair  of 
birthtime/death-time for the contact by pointing to a curve or table.  These pairs 
can  be  unique  for  the  dynamic  relaxation  phase  and  the  normal  phase  of  the 
simulation. 
•  Add  EDGEONLY  option  to  *CONTACT_AUTOMATIC_GENERAL  to  exclude 
node-to-segment  contact  and  consider  only  edge-to-edge  and  beam-to-beam 
contact. 
•  VDC  defines  the  coefficient  of  restituion  when  variable  CORTYP  is  defined.  
*CON-
Available 
TACT_AUTOMATIC_SURFACE_TO_SURFACE,  and  *CONTACT_AUTOMAT-
IC_SINGLE_SURFACE; SOFT = 0 or 1 only. 
*CONTACT_AUTOMATIC_NODES_TO_SURFACE, 
for 
•  Enhancements for *CONTACT_AUTOMATIC_GENERAL: 
◦  Add  beam  to  beam  contact  option  CPARM8  in  *PART_CONTACT  (MPP 
only). 
◦  Add option whereby beam generated on exterior shell edge will be shifted 
into  the  shell  by  half  the  shell  thickness.    In  this  way,  the  shell-edge-to-
shell-edge  contact  starts  right  at  the  shell  edge  and  not  at  an  extension  of 
the shell edge . 
•  Implement *CONTROL_CONTACT PENOPT = 3 option to *CONTACT_AUTO-
*CONTACT_ERODING_NODES_TO_-
MATIC_NODES_TO_SURFACE  and 
SURFACE for SMP. 
•  Update  segment  based  (SOFT = 2)  contact  to  improve  accuracy  at  points  away 
from  the  origin.    The  final  calculations  are  now  done  with  nodal  and  segment 
locations that have been shifted towards the origin so that coordinate values are 
small. 
•  Enable user defined friction (*USER_INTERFACE_FRICTION; subroutine usrfrc) 
for MPP contact SOFT = 4.
INTRODUCTION 
•  Unify automatic tiebreak messages for damage start and final failure.  SMP and 
MPP  should  now  give  the  same  output  to  d3hsp  and  messag.    This  affects 
*CONTACT_AUTOMATIC_...TIEBREAK, OPTIONs 6, 7, 8, 9, 10, and 11. 
•  *CONTACT_ADD_WEAR:  Associates  wear  calculations  to  a  forming  contact 
interface whose quantities can be posted in the intfor database file.  Adaptivity is 
supported. 
•  *CONTACT_..._MORTAR: 
◦  Detailed warning outputs activated for mortar contact, also clarifies echoed 
data in d3hsp. 
◦  Contact thickness made consistent with other contacts in terms of priority 
between ISTUPD on CONTROL_SHELL, SST on CONTACT and OPTT on 
PART_CONTACT. 
◦  Efficency improvement of bucket sort in mortar contact allowing for signif-
icant speedup in large scale contact simulations. 
•  *CONTACT_..._MORTAR, *DEFINE_FRICTION, *PART_CONTACT: 
◦  Mortar  contact  supports  FS = -1.0,  meaning  that  frictional  coefficients  are 
taken from *PART_CONTACT parameters. 
◦  Mortar contact supports FS.EQ.-2 meaning that friction is taken from *DE-
FINE_FRICTION. 
•  *CONTACT_AUTOMATIC_SINGLE_SURFACE_MORTAR: 
IG-
NORE.LT.0  for  single  surface  mortar  contact  will  ignore  penetrations  of  seg-
ments that belong to the same part. 
Using 
•  Friction  factors  are  now  a  function  of  temperature  for  *CONTACT_..._THER-
MAL_FRICTION. 
•  *SET_POROUS_LAGRANGIAN:  new  keyword  to  define  the  porosity  of 
Lagrangian  elements  in  an  element  set.    The  porous  forces  are  computed  by 
*CONSTRAINED_LAGRANGE_IN_SOLID ctype = 11 or 12. 
•  *CONSTRAINED_LAGRANGE_IN_SOLID: CTYPE = 12 is now also available in 
2D. 
•  Add helix angle option for *CONSTRAINED_JOINT_GEARS. 
•  Change keyword from *CONSTRAINED_BEARING to *ELEMENT_BEARING. 
•  Enhance  explicit  to  use  the  implicit  inertia  relief  constraints.    This  allows 
implicit-explicit switching for such problems. 
•  Add new input options to *CONTROL_IMPLICIT_INERTIA_RELIEF. 
◦  user specified number of nodes 
◦  user specified list of modes to constrain out.
INTRODUCTION 
•  Implement  *CONSTRAINED_BEAM_IN_SOLID.    This  feature  is  basically  an 
overhauled  constraint  couping  between  beams  and  Lagrangian  solids  that  in-
cludes  features  that  make  it  more  attractive  in  some  cases  than  *CON-
STRAINED_LAGRANGE_IN_SOLID,  for  example,  in  modeling  coupling  of 
rebar in concrete. 
•  Allow  *CONSTRAINED_INTERPOLATION  to  use  node  set  to  define  the 
independent nodes. 
•  Add  new  feature  MODEL.GE.10  to  *CONSTRAINED_INTERPOLATION_-
SPOTWELD  (SPR3).   This  allows  parameters  STIFF,  ALPHA1,  RN,  RS,  and  BE-
TA  to  be  defined  as  *DEFINE_FUNCTIONs  of  thicknesses  and  maximum 
engineering yield stresses of connected sheets. 
•  Add failure reports for *CONSTRAINED_SPR2. 
•  Add  more  d3hsp  output  for  *CONSTRAINED_INTERPOLATION_SPOTWELD 
and  *CONSTRAINED_SPR2.    Can  be  deactivated  by  setting  NPOPT = 1  on 
*CONTROL_OUTPUT. 
•  Add  option  to  *CONSTRAINED_JOINT:  Relative  penalty  stiffness  can  now  be 
defined  as  function  of  time  when  RPS < 0  refers  to  a  load  curve.    Works  for 
SPHERICAL, REVOLUTE, CYLINDRICAL in explixit analyses. 
•  Variable  MODEL  invokes  new  SPR4  option  in  *CONSTRAINED_INTERPOLA-
TION_SPOTWELD. 
•  *CONSTRAINED_JOINT_GEARS:  Gear  joint  now  supports  bevel  gears  and 
similar  types,  i.e.,  the  contact  point  does  not  necessarily  have  to  be  on  the  axis 
between the gear centers. 
•  *CONSTRAINED_MULTIPLE_GLOBAL:  Support  multiple  constraints  defined 
on the extra DOFs of user-defined elements. 
•  Make  the  *CONTROL_SHELL  PSNFAIL  option  work  with  the  W-MODE 
deletion criterion for shells. 
•  New  subcycling  scheme  activated  for  *CONTROL_SUBCYCLE  and  *CON-
TROL_SUBCYCLE_MASS_SCALED_PART.    By  default  the  ratio  between  the 
largest  and  smallest  time  step  is  now  16  and  the  external  forces  are  evaluated 
every time step.  The old scheme had a hard wired ratio of 8.  The ratios can be 
optionally  changed  by  *CONTROL_SUBCYCLE_K_L  where  K  is  the  maximum 
ratio between time steps for internal forces and L is likewise the ratio for external 
forces. 
•  *DATABASE_PROFILE: 
◦  output kinetic and internal energy profiles, 
◦  output volume fraction profiles, 
◦  add  a  parameter  MMG  to  specify  the  ALE  group  for  which  element  data 
can be output.
INTRODUCTION 
•  *DATABASE_ALE_MAT:  can  now  use  *DEFINE_BOX  to  compute  the  material 
energies,  volumes  and  masses  for  elements  inside  boxes  (instead  of  the  whole 
mesh). 
•  *DATABASE_TRACER_GENERATE:  new  keyword  to  create  ALE  tracer 
particles along iso-surfaces. 
•  *DATABASE_FSI:  add  option  to  output  moments  created  by  FSI  forces  about 
each node in a node set.  These moments about nodes are reported in dbfsi. 
•  Add  *DATABASE_BEARING  to  write  brngout  data  pertaining  to  *ELEMENT_-
BEARINGs. 
•  Include  eroded  hourglass  energy  in  hourglass  energy  in  glstat  file  to  be  con-
sistent  with  KE  &  IE  calculations  so  that  the  total  energy = kinetic  energy  + 
internal energy + hourglass energy + rigidwall energy. 
•  Add support for new database pbstat (*DATABASE_PBSTAT) for *PARTICLE_-
BLAST. 
◦  internal energy and translational energy of air and detonation products 
◦  force/pressure of air and detonation products for each part 
•  *DATABASE_EXTENT_INTFOR:    New  parameter  NWEAR  on  optional  card 
governs the output of wear depth to the intfor database. 
•  Using  CMPFLG = -1  in  *DATABASE_EXTENT_BINARY  will  work  just  as 
CMPFLG = 1, except that for *MAT_FABRIC (form 14 and form -14) and *MAT_-
FABRIC_MAP  the  local  strains  and  stresses  will  be  engineering  quantities  in-
stead of Green-Lagrange strain and 2nd Piola-Kirchhoff stress. 
•  For  some  materials  and  elements,  thermal  and  plastic  strain  tensors  can  be 
output to d3plot database, see STRFLG in *DATABASE_EXTENT_BINARY. 
•  Add  option  for  output  of  detailed  (or  long)  warning/error  messages  to  d3msg.  
See  MSGFLG  in  *CONTROL_OUTPUT.    Only  a  few  "long"  versions  of  warn-
ings/errors at this time but that list is expected to grow. 
•  Add two new options for rigid body data compression in d3plot; see DCOMP in 
*DATABASE_EXTENT_BINARY. 
•  Add option to write revised legend to jntforc, secforc, rcforc, deforc and nodout 
files  via  input  flag  NEWLEG  in  *CONTROL_OUTPUT.    This  helps  to  avoid 
confusion over unassigned IDs and duplicated IDs. 
•  If any input data is encrypted and dynain is requested, the code issues an error 
message and stops the job. 
•  Solid  part  or  solid  part  set  is  now  allowed  for  *DEFINE_DE_TO_SURFACE_-
COUPLING. 
•  Implement *DELETE_PART for Discrete Element Sphere.
INTRODUCTION 
•  The  unit  of  contact  angle  changed  from  radian  to  degree  for  *CONTROL_DIS-
CRETE_ELEMENT. 
•  Implement Archard's wear law to *DEFINE_DE_TO_SURFACE_COUPLING for 
discrete element spheres.  Wear factor is output to DEM binout database. 
•  Add  damping  energy  and  frictional  energy  of  discrete  elements  to  "damping 
energy" and "sliding interface energy" terms in glstat. 
•  Introduce a small perturbation to the initial position of newly generated discrete 
elements  for  *DEFINE_DE_INJECTION.    This  allows  a  more  random  spatial 
distribution of the generated particles. 
•  *INTERFACE_DE_HBOND  replaces  *INTERFACE_DE_BOND.    Used  to  define 
the  failure  models  for bonds  linking  various discrete  element (DE) parts  within 
one heterogeneous bond definition (*DEFINE_DE_HBOND). 
•  *DEFINE_ADAPTIVE_SOLID_TO_DES:  Embed  and/or  transform  failed  solid 
elements to DES (*ELEMENT_DISCRETE_SPHERE) particles.  The DES particles 
inherit the material properties of the solid elements.   All DES-based features are 
available  through  this  transformation,  including  the  bond  models  and  contact 
algorithms.    This  command  is  essentially  to  DES  what  *DEFINE_ADAPTIVE_-
SOLID_TO_SPH is to SPH particles. 
•  Add EM orthotropic materials where the electric conductivity is a 3x3 tensor, see 
new card, *EM_MAT_003. 
•  Add new keyword family, *EM_DATABASE_...  which triggers the output of EM 
quantites  and  variables.    All  EM  related  ASCII  outputs  now  start  with  em_***.  
Keywords are : 
◦    EM_DATABASE_CIRCUIT 
◦    EM_DATABASE_CIRCUIT0D 
◦    EM_DATABASE_ELOUT 
◦    EM_DATABASE_GLOBALENERGY 
◦    EM_DATABASE_NODOUT 
◦    EM_DATABASE_PARTDATA 
◦    EM_DATABASE_POINTOUT 
◦    EM_DATABASE_ROGO 
◦    EM_DATABASE_TIMESTEP 
•  Add capability to plot magnetic field lines in and around the conductors at given 
times,  see  *EM_DATABASE_FIELDLINE.    ASCII  output  files  are  generated 
(lspp_fieldLine_xx) and are readable by LSPP in order to plot the field lines.  In 
the future, LSPP will be capable of directly generating the field lines. 
•  Add EM quantities in *DEFINE_CURVE_FUNCTION: 
◦   EM_ELHIST for element history (at element center). 
◦   EM_NDHIST for node history.
INTRODUCTION 
◦  EM_PAHIST for part history (integrated over the part). 
•  Add  *EM_EOS_TABULATED2  where  a  load  curve  defines  the  electrical 
conductivity vs time. 
•  Introduce  capability  to  use  the  EM  solver  on  (thin)  shells:  An  underlying  solid 
mesh (hexes and prisms) is  built where the EM is  solved and the EM fields are 
then collapsed onto the corresponding shell.  The EM mat for shells is defined in 
*EM_MAT_004.    This  works  for  EM  solvers  1,  2  and  3  and  the  EM  contact  is 
available for shells. 
•  Add different contact options in the *EM_CONTACT card. 
•  Add  new  methods  to  calculate  electric  contact  resistance  between  two  conduc-
tors  for  Resistive  Spot  Welding  applications  (RSW).    See  *EM_CONTACT_RE-
SISTANCE. 
•  Add  Joule  Heating  in  the  contact  resistance  (*EM_CONTACT_RESISTANCE).  
The Joule heating is evenly spread between the elements adjacent to the faces in 
contact. 
•  Add  new  circuit  types  21  and  22    allowing  users  to  put  in 
their own periodic curve shape when using the inductive heating solver.  This is 
useful in cases where the current is not a perfect sinusoidal. 
•  Provide  default  values  for  NCYCLEBEM  and  NCYCLEFEM  (=5000)  and  set 
default value of NUMLS to 100 in *EM_CIRCUIT. 
•  Add two additional formulations, FORM = 3 and 4, to *PART_MODES. 
•  Add 20-node solid element, ELFORM = 23 in *SECTION_SOLID. 
•  Add  H8TOH20  option  to  *ELEMENT_SOLID  to  convert  8-node  to  20-node 
solids. 
•  Add  option  SOLSIG  to  *CONTROL_OUTPUT  which  will  permit  stresses  and 
other  history  variables  for  multi-integration  point  solids  to  be  extrapolated  to 
nodes.      These  extrapolated  nodal  values  replace  the  integration  point  values 
normally  stored  in  d3plot.    NINTSLD  must  be  set  to  8  in  *DATABASE_EX-
TENT_BINARY when a nonzero SOLSIG is specified.  Supported solid formula-
tions are solid elements are: -1, -2, 2, 3, 4, 18, 16, 17, 23. 
•  Activate contact thickness input from *PART_CONTACT for solids. 
•  Made  many  enhancements  for  *PART_MODES  for  robustness  and  MPP 
implementation. 
•  Add  new  cohesive  shell  element  (elform = 29)  for  edge-to-edge  connectivity 
between shells.  This element type takes bending into account and supports MPP 
and implicit solvers. 
•  Error terminate with message, STR+1296, if same node is defined multiple times 
in *ELEMENT_MASS_MATRIX.
INTRODUCTION 
•  Add  support  for  negative  MAXINT  option  in  *DATABASE_EXTENT_BINARY 
for thick shell elements. 
•  *ELEMENT_TSHELL:  Add  "BETA"  as  option  for  *ELEMENT_TSHELL  to 
provide an orthotropic material angle for the element. 
•  Add  Rayleigh  damping  (*DAMPING_PART_STIFFNESS)  for  triangular  shell 
element types 3 and 17. 
•  Add  new  keyword  *ELEMENT_BEAM_SOURCE.    Purpose:    Define  a  nodal 
source for beam elements.  This feature is implemented for truss beam elements 
(ELFORM = 3)  with  material  *MAT_001  and  for  discrete  beam  elements 
(ELFORM = 6) with material *MAT_071. 
•  Add new option to *DEFINE_ELEMENT_DEATH.  New variable IDGRP defines 
a group id for simultaneous deletion of elements. 
•  Convert  cohesive  solid  type  20  and  22  to  incremental  formulation  to  properly 
handle large rotations.  Also use consistent mass. 
•  Add Smoothed Particle Galerkin (SPG) method for solid analysis (ELFORM = 47) 
and  corresponding  keyword  option  *SECTION_SOLID_SPG.    SPG  is  a  true 
particle  method  in  Galerkin  formulation  that  is  suitable  for  severe  deformation 
problems and damage analysis. 
•  Enhance  *ELEMENT_LANCING  by  supporting  *PARAMETER,  *PARAME-
TER_EXPRESSION. 
•  Add  a  new  feature,  *CONTROL_FORMING_TRIMMING,  for  2D  and  3D 
trimming of a 3-layer, sandwich laminate blank via *DEFINE_CURVE_TRIM. 
•  Add 3D normal trimming of solid elements via *DEFINE_CURVE_TRIM_3D. 
•  Add  new  features  for  solid  elements  2D  trimming  *DEFINE_CURVE_TRIM_-
NEW: 
◦  Allow  support  of  arbitrary  trimming  vector  (previously  only  global  z  di-
rection was allowed). 
◦  Improve trimming algorithm for speed up. 
◦  Allow trimming curves to project to either the top or bottom surface. 
•  Add a new AUTO_CONSTRAINT option to *CONTROL_FORMING_ONESTEP 
which is convenient for blank nesting. 
•  Add  new  features  to  *CONTROL_FORMING_SCRAP_FALL.    Previously  the 
user  was  required  to  define  the  trimmed  blank  properly.    Now  the  blank  is 
trimmed by the cutting edge of the trim steel, which is defined by a node set and 
a moving vector. 
•  Enhance  *CONTROL_FORMING_SCRAP_FALL:  Allow  the  node  set  (NDSET) 
on the trim steel edge to be defined in any order. 
•  Improve *CONTROL_FORMING_ONESTEP:
INTRODUCTION 
◦  Reposition the initial part before unfolding, using the center element nor-
mal. 
◦  Add a message showing that the initial unfolding is in process. 
•  Add  2D  trimming  for  solid  elements  *DEFINE_CURVE_TRIM_NEW,  support 
*DEFINE_TRIM_SEED_POINT_COORDINATES. 
•  Add *CONTROL_FORMING_AUTOCHECK to detect and fix flaws in the mesh 
for the rigid body that models the tooling. 
•  Add new features to *CONTROL_FORMING_UNFLANGING: 
◦  The incoming flange mesh will be automatically checked for mesh quality 
and bad elements fixed. 
◦  Allow thickness offset of deformable flange to use the blank thickness from 
user's input. 
◦  Allow definition any node ID in the outer boundary of the flange, to speed 
up the search when holes are present in the part. 
◦  Add a new parameter CHARLEN to limit the search region. 
◦  Allow holes to exist in the flange regions. 
◦  Output a suggested flange part after unflanging simulation, with the failed 
elements deleted from the unflanged part. 
◦  Automatically  define  a  node  set  and  constraints  for  the  flange  boundary 
nodes through the user definition of three nodes. 
◦  Add output of forming thickness, effective strain and trim curves after un-
flanging simulation. 
•  Add  a  new  keyword  *CONTROL_FORMING_TRIM  to  replace  *ELEMENT_-
TRIM. 
•  Add a new keyword: *CONTROL_FORMING_UNFLANGING_OUTPUT: Failed 
elements are removed to come up with the trim curves. 
•  Add  new  features  to  *INTERFACE_BLANKSIZE_DEVELOPMENT  including 
allowing for trimming between initial and final blank. 
•  Enhance *CONTROL_FORMING_OUTPUT for controlling the number of states. 
•  Add  *CONTROL_FORMING_TRIM_MERGE  to  close  a  user  specified  (gap) 
value  in  the  trim  curves,  so  each  trim  curve  will  form  a  closed  loop,  which  is 
required for a successful trimming. 
•  Add  *CONTROL_FORMING_MAXID  to  set  a  maximum  node  ID  and  element 
ID for the incoming dynain file (typically the blank) in the current simulation. 
•  Enhance *FREQUENCY_DOMAIN_ACOUSTIC_BEM: 
◦  Update  the  boundary  condition  definition  for  BEM  acoustics  so  that  im-
pedance  and  other  user  defined  boundary  conditions  can  be  combined 
with time domain velocity boundary condition.
INTRODUCTION 
◦   Implement Burton-Miller BEM to MPP. 
◦  Implement impedance boundary condition to Burton-Miller BEM. 
◦  Implement  half  space  option  (*FREQUENCY_DOMAIN_ACOUSTIC_-
BEM_HALF_SPACE) to  variational indirect BEM. 
◦  Implement half space option to acoustic scattering problems. 
◦  Extend acoustic ATV computation to elements, in addition to nodes. 
◦  Support element based ATV output in d3atv. 
◦  Add an option (_MATV) to run modal acoustic transfer vector.  Implement 
MATV to MPP. 
◦  Implement  running  BEM  Acoustics  based  on  modal  ATV  (SSD  excitation 
only). 
•  *FREQUENCY_DOMAIN_ACOUSTIC_FEM:    Enable  running  FEM  acoustics 
based on restarting SSD (*FREQUENCY_DOMAIN_SSD). 
•  Add  *FREQUENCY_DOMAIN_ACOUSTIC_INCIDENT_WAVE  to  define  the 
incident  waves  for  acoustic  scattering  problems.    To  be  used  with  *FREQUEN-
CY_DOMAIN_ACOUSTIC_BEM. 
•  Add  *FREQUENCY_DOMAIN_ACOUSTIC_SOUND_SPEED  to  define  frequen-
cy  dependent  complex  sound  speed,  which  can  be  used  in  BEM  acoustics.    By 
using complex sound speed, the damping in the acoustic system can be consid-
ered.  To be used with *FREQUENCY_DOMAIN_ACOUSTIC_BEM. 
•  *FREQUENCY_DOMAIN_FRF:  Add  mode  dependent  rayleigh  damping  to  frf 
and ssd (DMPMAS and DMPSTF). 
•  *FREQUENCY_DOMAIN_RESPONSE_SPECTRUM: 
◦  Add output of nodout_spcm and elout_spcm, to get nodal results and ele-
ment results at user specified nodes and elements. 
◦  Add von Mises stress computation. 
•  *FREQUENCY_DOMAIN_RANDOM_VIBRATION:  Add  semi-log,  and  linear-
linear interpolation on PSD curves (parameter LDFLAG). 
•  *FREQUENCY_DOMAIN_SSD: 
◦  Add strain computation. 
◦  Add parameter LC3 to define the duration of excitation for each frequency. 
◦  Implement fatigue analysis option (_FATIGUE) based on ssd (sine sweep). 
◦  Add  option  to  use  *DAMPING_PART_MASS  and  *DAMPING_PART_-
STIFFNESS in SSD (DMPFLG = 1). 
•  Add  *MAT_ADD_FATIGUE  to  define    material's  SN  fatigue  curve  for  applica-
tion in vibration fatigue and SSD fatigue analysis. 
•  Add 
*FREQUENCY_DOMAIN_ACCELERATION_UNIT 
to 
facilitate 
the 
acceleration unit conversion.
INTRODUCTION 
•  The  icfd_mstats.dat  file  now  outputs  the  ten  worst  quality  element  locations 
(ICFD solver). 
•  Add  option  in  *ICFD_CONTROL_OUTPUT  allowing  terminal  output  to  be 
written to messag file. 
•  Add keyword *ICFD_CONTROL_OUTPUT_SUBDOM to output only part of the 
domain.  Available for vtk, dx and gmv formats. 
•  Add  new  keyword  family,  *ICFD_DATABASE_...    which  triggers  the  output  of 
ICFD variables.  All ICFD related output files now start with icfd_***. 
•  Add  new  keyword  family  *ICFD_SOLVER_TOL_...    which  allows  the  user  to 
control  tolerances  and  iteration  number  for  the  fractional  step  solve,  the  mesh 
movement solve, and the heat equation solve. 
•  Curves in *ICFD_BOUNDARY_PRESCRIBED_VEL each provide a scaling factor 
vs.    x,y,  or  z  coordinate,  respectively.    These  scaling  factors  are  applied  to  the 
velocity boundary condition. 
•  Enable free-slip condition for FSI walls (ICFD solver). 
•  Add new variable IDC to *ICFD_CONTROL_FSI that allows the modification of 
the scaling parameter that multiplies the mesh size to detect contact. 
•  Add  automatic  squeezing  to  the  ICFD  elements  of  the  boundary  layer  when 
there are two very close surfaces with poor (coarse) mesh resolution. 
•  Add the initialization for all nodes using *ICFD_INITIAL with PID = 0. 
•  Add  a  curve  (LCIDSF  in  *ICFD_CONTROL_TIME)  that  scales  the  CFL  number 
as a function of time. 
•  Add  a  Heaviside  function  that  allows  the  solution  of  simple  multiphase 
problems (ICFD). 
•  Add the computation of the heat convection coefficient (ICFD). 
•  Add MPP support for y+ and shear for output (ICFD). 
•  Add uniformity index (ICFD). 
•  Add  *ICFD_CONTROL_TAVERAGE  to  control  the  restarting  time  for  compu-
ting the time average values. 
•  Implement the XMl format for vtk.  See *ICFD_CONTROL_OUTPUT. 
•  Improve temperature stabilization for thermal problems (ICFD). 
•  Add the Generalized Flow Through Porous Media model monolithically coupled 
to  the  incompressible  Navier-Stokes  model.    See  keyword  *ICFD_MAT  for  the 
new options. 
•  Add  the  Anisotropic  version  of  the  Generalized  Flow  in  Porous  Media.    See 
*ICFD_MAT for details.
INTRODUCTION 
•  Add  the  capability  to  define  the  porous  properties  using  the  Pressure-Velocity 
(P-V) experimental curves.  See *ICFD_MAT. 
•  Compute drag forces around anisotropic/isotropic porous domains (ICFD). 
•  Extend  implicit  debug  checking  when  LPRINT = 3  on  *CONTROL_IMPLICIT_-
SOLVER. 
•  Add option for implicit dynamic relaxation so that only a subset of parts is active 
during the dynamic relaxation phase. 
•  Extend implicit time step control via  IAUTO < 0 in *CONTROL_IMPLICIT_AU-
TO to linear analysis. 
•  Add  self  piercing  rivet  capability  to  implicit  (*CONSTRAINED_SPR2,  *CON-
STRAINED_INTERPOLATION_SPOTWELD). 
•  Add  MTXDMP  in  *CONTROL_IMPLICIT_SOLVER  to  dump  the  damping 
matrix from implicit mechanics. 
•  Improve stress and strain computation induced by mode shapes.  See  MSTRES 
in *CONTROL_IMPLICIT_EIGENVALUE. 
•  Add  variable  MSTRSCL  to  *CONTROL_IMPLICIT_EIGENVALUE  for  user 
control of geometry scaling for the stress computation. 
•  Make SMP and MPP treatment of autospc constraints consistent.  See AUTOSPC 
on *CONTROL_IMPLICIT_SOLVER. 
•  Enhance  output  for  *ELEMENT_DIRECT_MATRIX_INPUT  (superelements)  to 
describe how they are attached to the LS-DYNA model. 
•  Enhance superelement computation (*CONTROL_IMPLICIT_MODES or *CON-
TROL_IMPLICIT_STATIC_CONDENSATION): 
◦  The computation of the inertia matrix in the presense of rigid bodies is cor-
rect. 
◦  Adjust superelement computation to accept initial velocities. 
◦  Add null beams for the visualization of superelements. 
•  Enhance  implicit  to  allow  the  use  of  *CONSTRAINED_RIVET  in  conjunction 
with axisymmetric shell element problems. 
•  Add  output  of  performance  statistics  for  the  MPP  implicit  eigensolver  to 
mes0000. 
•  Add Stress computation to modal dynamics (*CONTROL_IMPLICIT_MODAL_-
DYNAMIC). 
•  Allow  unsymmetric  terms  to  the  assembled  stiffness  matrix  from  some  implicit 
features.
INTRODUCTION 
•  Enhance  implicit-explicit  switching  (IMFLAG < 0  in  *CONTROL_IMPLICIT_-
GENERAL) so that curve |IMFLAG| can be defined using *DEFINE_CURVE_-
FUNCTION. 
•  Upgrade the implicit implementation of rack and pinion and screw joints so the 
joint is driven by relative motion of the assembly instead of absolute motion. 
•  Add *CONTACT_1D to implicit mechanics. 
•  *CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS 
Rotordynamics using the implicit time integrator. 
is 
added 
to 
study 
•  *MAT_SEATBELT is supported for implicit by introducing bending stiffness. 
•  *INITIAL_LAG_MAPPING  added  to  initialize  a  3D  Lagrangian  mesh  from  the 
last cycle of a 2D Lagrangian simulation. 
•  *ELEMENT_SHELL_NURBS_PATCH: 
◦  Add support for dumping of strain tensor and shell internal energy densi-
ty for isogeometric shells via interpolation shells. 
◦  Add conventional mass-scaling for isogeometric shells. 
•  *LOAD_BODY_POROUS: applies also now to 1D and 2D problems. 
•  Add  *LOAD_SEGMENT_CONTACT_MASK,  which  currently  works  in  MPP 
only.  This feature masks the pressure from a *LOAD_SEGMENT_SET when the 
pressure segments are in contact with another material. 
•  Curve  LCID  of  *LOAD_NODE  can  be  defined  by  *DEFINE_CURVE_FUNC-
TION. 
•  *USER_LOADING:  pass  more  data  to  user-defined  loading  subroutine  loadud 
including nodal moment, nodal rotational displacement and velocity, and  nodal 
translational mass and rotational inertia. 
•  Add load curves for dynamic relaxation for *LOAD_THERMAL_VARIABLE. 
•  *LOAD_SEGMENT_NONUNIFORM, 
*LOAD_SEGMENT_SET_NONUNI-
FORM:  By  specifying  a  negative  load  curve  ID  the  applied  load  becomes  a 
follower  force,  i.e.,  the  direction  of  the  load  is  constant  with  respect  to  a  local 
coordinate system that rotates with the segment. 
•  Make several enhancements to *MAT_172. 
•  *MAT_HYPERELASTIC_RUBBER  (*MAT_077_H)  has  new  thermal  option  for 
material properties. 
•  Add 
*MAT_ORTHOTROPIC_PHASE_CHANGE, 
*MAT_ELASTIC_PHASE_-
CHANGE, and 
•  *MAT_MOONEY-RIVLIN_PHASE_CHANGE  whereby  elements  change  phase 
as they cross a plane in space.
INTRODUCTION 
•  Add P1DOFF to 2D seatbelt material, *MAT_SEATBELT_2D, to specify a part ID 
offset for the internally created 1D seatbelt elements. 
•  All load curves for *MAT_067 can be defined via *DEFINE_FUNCTION. 
•  Enhance *MAT_CWM: 
◦  Add support for shell elements. 
◦  Add  support  for  hardening  curves.    Yield  stress  can  be  supplied  as  table 
depending on plastic strain and temperature. 
•  Check  diagonal  elements  of  C-matrix  of  *MAT_002/MAT_{OPTION}TROPIC_
ELASTIC and error terminate with message, STR+1306, if any are negative. 
•  Add a keyword option called MIDFAIL for *MAT_024, (MAT_PIECEWISE_LIN-
EAR_PLASTICITY).  When MIDFAIL appears in the keyword, failure by plastic 
strain  will  only  be  checked  at  the  mid-plane.    If  the  mid-plane  fails,  then  the 
element  fails.    If  there  are  an  even  number  of  integration  points  through  the 
thickness, then the two points closest to the middle will check for failure and the 
element fails when both layers fail. 
•  Enable solid and solid assembly spot welds (*MAT_SPOTWELD) to use the NF 
parameter for force filtering. 
•  Add  the  shear  angle  in  degrees  as  the  first  history  variable  for  shell  material 
*MAT_214 (DRY_FABRIC). 
•  Expand from 2 to 5 the number of additional cards that can be used for the user 
defined weld failure, OPT = 12 or OPT = 22 on *MAT_SPOTWELD.  Now a total 
of 46 user variables are possible. 
•  Add  a  solid  spot  weld  material  option  in  *MAT_SPOTWELD  to  treat  the  stress 
state as uniaxial.  This option is available for solid assemblies also. 
•  Add *MAT_FABRIC form 24 which is a modified version of form 14.  The main 
improvement  is  that  the  Poisson's  effects  work  correctly  with  the  nonlinear 
curves  for  fiber  stress.    Also,  the  output  of  stress  and  strain  to  d3plot  are  engi-
neering stress and strain instead of 2nd PK stress and Green's strain.  Added an 
option to input curves in engineering stress and strain rather than 2nd PK stress 
vs.  Green's strain.  To use this, set DATYP = -2 on *DEFINE_CURVE. 
•  Increase maximum number of plies from 8 to 24 in a sublaminate with *MAT_-
CODAM2. 
•  Add *MAT_THERMAL_CHEMICAL_REACTION to model a material undergo-
ing  a  chemical  reaction  such  as  an  epoxy  used  in  manufacturing  composite 
materials. 
•  *MAT_058: 
◦  Add  option  to  use  nonlinear  (elastic)  stress-strain  curves  instead  of  con-
stant stiffnesses (EA, EB, GAB).
INTRODUCTION 
◦  Add  option  to  use  strain-rate  dependent  nonlinear  (elastic)  stress-strain 
curves instead of constant stiffnesses (EA, EB, GAB). 
◦  Add option to define proper poisson ratios PRCA and PRCB (also added in 
*MAT_158). 
•  Add  option  to  use  yield  curve  or  table  in  *MAT_100  (*MAT_SPOTWELD)  for 
solid elements. 
•  Add *MAT_157 for solid elements.  This includes an optional variable IHIS that 
invokes  *INITIAL_STRESS_SOLID  to  initialize  material  properties  on  an  ele-
ment-by-element  basis.    This  was  developed  to  allow  a  user  to  map/initialize 
anisotropic material properties from an injection molding simulation. 
•  *MAT_157 (shells): 
◦  Add anisotropic scale factor for plastic strain rate (VP = 1 only). 
◦  Improve local stress projection for VP = 1. 
◦  Add optional variable IHIS, similar to that described for solids above. 
•  Add  strain  rate  dependence  to  *MAT_103  for  solids  via  a  table  (isotropic 
hardening only). 
•  *MAT_136  (*MAT_CORUS_VEGTER):  Implemented  an  alternative,  implicit 
plasticity algorithm (define N.lt.0) for enhanced stability. 
•  *MAT_244 (*MAT_UHS_STEEL): 
◦  In plasticity with non-linear hardening, temperature effects and strain rate 
effects are now dealt with the same way they are implemented in *MAT_-
106.  In particular, strain rate now refers to the plastic strain rate. 
◦  Allow  for  the  definition  of  start  temperatures  for  each  phase  change,  for 
cooling and heating. 
◦  Account  for  elastic  transformation  strains,  given  as  a  curve  wrt  tempera-
ture. 
◦  Add feature to *MAT_244 for welding simulations.  Similar to *MAT_270, 
material  can  be  initialized  in  a  quiet  (ghost)  state  and  activated  at  a  birth 
temperature. 
•  Furthermore, annealing is accounted for. 
•  - Modify formula for Pearlite phase kinetics based on Kirkaldy and Venugoplan 
(1983). 
•   
•  *MAT_249 
(*MAT_REINFORCED_THERMOPLASTIC): 
Implement 
new 
material formulation for shells, which is based on additive split of stress tensor.
INTRODUCTION 
◦  For  the  thermoplastic  matrix,  a  thermo-elasto-plastic  material  is  imple-
load 
temperature  dependence 
is  defined  by 
mented,where 
curves/tables in the input file. 
the 
◦  Includes hyperelastic fiber contribution. 
◦  For any integration point, up to three different fiber directions can be de-
fined.    Their  (non-linear)  response  to  elongation  and  shear  deformations 
can also be defined with load curves. 
◦  Includes input parameters for anisotropic transverse shear stiffness. 
•  *MAT_T07  (*MAT_THERMAL_CWM):  Add  HBIRTH  and  TBIRTH  which  are 
specific heat and thermal conductivity, resp., used for time t < TISTART. 
•  One additional parameter (exponent GAMMA) for B-K law of *MAT_138. 
•  MAT_187: Speed-up of load curve lookup for curves with many points. 
•  Add  new  option  "MAGNESIUM"  to  *MAT_233.    Differences  between  tension 
and compression are included. 
•  Add enhanced damage model with crack closure effects to *MAT_104. 
•  Some  improvements  for  *MAT_075  (BILKHU/DUBOIS_FOAM):  Volumetric 
strain  rate  can  now  be  averaged  over  NCYCLE  cycles,  original  input  curve 
LCRATE is instead of a rediscretized curve, and averaged strain rate is stored as 
history variable #3. 
•  Add  new  history  variables  to  *MAT_123:    A  mixed  failure  indicator  as  history 
variable #10 and triaxiality as #11. 
•  Decrease memory requirements for *MAT_ADD_EROSION by 50%. 
•  Add *MAT_098 for tetrahedral solid type 13. 
•  Add  new  history  variable  #8  to  *MAT_157  for  shell  elements:  "Anisotropic 
equivalent plastic strain". 
•  Add  tangent  stiffness  to  *MAT_224  for  implicit  analyses  with  solid  and  shell 
elements. 
•  Put internal enery on "plastic strain" location for *MAT_027 solids. 
•  Add  new  option  *MAT_224:  BETA  .LT.    0:  strain  rate  dependent  amount  given 
by load curve ID = -BETA 
•  Add new flag to switch off all MAT_ADD_EROSION definitions globally. 
•  This will be the 1st parameter "MAEOFF" on new keyword *CONTROL_MAT. 
•  Add option to define a load curve for isotropic hardening in *MAT_135. 
•  *MAT_CDPM  is  reimplemented  by  its  original  developers  (Peter  Grassl  and 
Dimitros  Xenos  at  University  of  Glasgow)  for  enhanced  robustness.    A  new 
parameter EFC is introduced governing damage in compression and the bilinear 
law is exchanged for an exponential one.
INTRODUCTION 
•  *MAT_3-PARAMETER_BARLAT:    HR = 7  is  complemented  with  biaxial/shear 
hardening curves. 
•  *MAT_FABRIC_MAP: 
◦  A stress map material for detailed stress response in fabrics, stress can be 
prescribed through tables PXX and PYY corresponding to functions of bi-
axial strain states. 
◦  A compaction effect due to packing of yarns in compression is obtained by 
specifying BULKC (bulk modulus) and JACC (critical jacobian for the on-
set  of  compaction  effect).    This  results  ib  increasing  pressure  that  resists 
membrane elements from collapsing and/or inverting. 
◦  Strain rate effects can be obtained by specifying FXX and FYY which in ef-
fect scales the stress based on engineering strain rate.  A smoothing effect 
is applied by using a time window DT. 
◦  A hysteresis option TH is implemented for stability, given in fraction dis-
sipated energy during a cycle.  Can also depend on the strain state through 
a table. 
•  *MAT_GENERAL_HYPERELASTIC_RUBBER, 
*MAT_OGDEN_RUBBER:  By 
specifying TBHYS.LT.0 a more intuitive interpolation of the damage vs.  devia-
toric  strain  energy  is  obtained.    It  requires  however  that  the  damage  and  strain 
energy axes are swapped. 
•  *MAT_SIMPLIFIED_RUBBER: For AVGOPT.LT.0 the absolute value represents a 
time  window  over  which  the  strain  rates  are  averaged.    This  is  for  suppressing 
extensive noise used for evaluating stress from tables. 
•  *MAT_FABRIC:  The  bending 
stiffness 
contribution 
in  material  34, 
ECOAT/SCOAT/TCOAT, is now supported in implicit calculations. 
•  Add *MAT_122_3D which is an extension of *MAT_122 to solid elements.  This 
material  model  combines  orthotropic  elastic  behavior  with  Hill’s  1948  aniso-
tropic plasticity theory and its applicability is primarily to composite materials. 
•  MPP groupable tied contact: Output messages about initial node movement due 
to projection like non-groupable routines do. 
•  MPP tied contact initialization: 
◦  Change a tolerance in groupable tied contact bucketsort to match the non-
groupable code, and fix the slave node thickness used for beam nodes dur-
ing initial search in non-groupable contact to match groupable contact. 
◦  Update the slave node from beam thickness calculation for type 9,11, and 
12 beams. 
•  For  MPP,  set  a  "last  known  location"  flag  to  give  some  indication  of  where  the 
processors were if an error termination happens.  Each writes a message to their
INTRODUCTION 
own  message  file.    Look  for  a  line  that  says  "When  error  termination  was  trig-
gered, this processor was". 
•  MPP  BEAMS_TO_SURFACE  contact:  Remove  "beam"  node  mass  from  the 
penalty stiffness calculation when soft = 1 is used, which matches SMP behavior. 
•  Make  sure  the  pfile.log  file  gets  created  in  case  of  termination  due  to  *CON-
TROL_STRUCTURED_TERM. 
•  Add two new decomposition region-related pfile options "nproc" and "%proc" so 
that  any  given  decomposition  region  can  be  assigned  to  some  subset  of  all  the 
processors.  nproc takes a single argument, which is a specific number of proces-
sors.  %proc takes a single argument, which is a percentage of processors to use.  
The old options "lump" and "distribute" are still available and are mapped to the 
new options thusly: 
◦  lump       => "nproc 1" 
◦  distribute => "%proc 100.0" 
•  Tweak MPP beam-to-beam contact routine for better handling of parallel beams. 
•  MPP: Add support for new solid and shell cost routines, invoked with the pfile 
option  "decomp  {  newcost  }".    Will  be  expanded  to  include  beams,  thick  shells, 
etc.  in the future. 
•  MPP  contact:  add  support  for  IGAP > 2  added  to  the  SINGLE_SURFACE,  AU-
TOMATIC_GENERAL, and *_TO_SURFACE contacts. 
•  Improve the way MPP computes slave node areas for AUTOMATIC_TIEBREAK 
contacts (and other that use areas).  This should result in less mesh dependency 
in the failure condition of AUTOMATIC_TIEBREAK contacts. 
•  MPP: synchronize rigid body flags for shared nodes during rigid-to-deformable 
switching so that these nodes are handled consistently across processors. 
•  Add new pfile decomposition region option “partsets”.  Takes a list of part sets 
(SET_PART) from the keyword input and uses them to define a region. 
•  Apply decomposition transformation (if defined) to: 
◦  *CONTROL_MPP_DECOMPOSITION_PARTS_DISTRIBUTE 
◦  *CONTROL_MPP_DECOMPOSITION_PARTSET_DISTRIBUTE 
◦  *CONTROL_MPP_DECOMPOSITION_ARRANGE_PARTS. 
•  Honor  TIEDPRJ  flag  on  *CONTROL_CONTACT  for  MPP  groupable  tied 
interfaces. 
•  Increase  initial  search  distance  in  MPP  tied  contact  to  include  slave  and  master 
thicknesses. 
•  Tweak MPP_INTERFERENCE contact to better handle deep initial penetrations.
INTRODUCTION 
•  MPP:  Reorganize  how  *RIGIDWALL_PLANAR_FORCES  is  handled,  which 
greatly improves scaling. 
•  Add  new  MPP  pfile  option:  directory  {  local_dirs  {  path1  path2  path3  }  which 
will assign different local working directories to different processors, to balance 
the I/O load. 
•  Miscellaneous MPP enhancements: 
◦  Restructure  and  reduce  memory  usage  of  3D  ALE  searching  of  neighbor-
ing  algorithm.    Now,  the  code  can  handle  hundreds  of  millions  ALE  ele-
ments during decomposition. 
◦  Support *PARTICLE_BLAST. 
◦  Support SPH 2D contact. 
◦  Greatly  speed  up  reconstruction  of  eroding  contact  surface,  (soft = 0,1) 
when using large number of cores. 
•  Add the following options for small restarts: 
◦  *CHANGE_VELOCITY_GENERATION, 
◦  *CHANGE_RIGIDWALL_option, 
◦  PSNFAIL option to *CONTROL_SHELL 
•  MPP  full  deck  restart:  Restore  behavior  consistent  with  SMP  which  is  that  only 
the nodes of materials being initialized (not all nodes) are initialized from d3full. 
•  MPP: add full deck restart support for AUTOMATIC_TIEBREAK contact types. 
•  Implement *DELETE_PART for seatbelt parts.  The associated slipring, retractors 
and pretensioners will be deactivated as well. 
•  Add support for MPP restarts with USA coupling. 
•  Add  NREP  option  to  *SENSOR_CONTROL  to  repeat  NREP  cycles  of  switches 
given on Card 2. 
•  Implement  *SENSOR_CONTROL  TYPEs    BELTPRET,  BELTRETRA  and  BELT-
SLIP control the pretensioners, retractors and sliprings of a 2D seatbelt. 
•  Add  function  SENSORD  to  *DEFINE_CURVE_FUNCTION  to  return  the  value 
of a sensor. 
•  Replace  *SENSOR_DEFINE_ANGLE  with  more  general  *SENSOR_DEFINE_-
MISC.  MTYPEs include ANGLE, RETRACTOR, RIGIDBODY, and TIME. 
•  Add rcforc output for *CONTACT_2D_NODE_TO_SOLID (supported for ASCII 
output only; not binout). 
•  Add temperature output (when applicable) to sphout file (*DATABASE_SPHO-
UT).
INTRODUCTION 
•  Add support of  *MAT_ALE_VISCOUS for SPH particles.  This allows modeling 
of non-viscous fluids with constant or variable viscosity, i.e, non-newtonian type 
fluid using SPH. 
•  Add support of *EOS for *MAT_272 with SPH particles. 
•  Add support of *MAT_255, *MAT_126, and *MAT_26 (with AOPT = 2 only) for 
SPH particles. 
•  Add new keyword command *SECTION_SPH_INTERACTION: Combined with 
CONT = 1  in  *CONTROL_SPH  card,  this  keyword  is  used  to  define  the  partial 
interaction between SPH parts through normal interpolation method and partial 
interaction  through  the  contact  option.    All  the  SPH  parts  defined  through  this 
keyword  will  interact  with  each  other  through  normal  interpolation  method 
automatically. 
•  Add  support  for  *DATABASE_TRACER  for  axisymmetric  SPH  (IDIM = -2  in 
*CONTROL_SPH). 
•  ICONT  in  *CONTROL_SPH  now  affects  *DEFINE_SPH_TO_SPH_COUPLING 
in the sense of enabling or disabling the coupling for deactivated particles. 
•  The  commands  *STOCHASTIC_TBX_PARTICLES  and  *CHEMISTRY_CON-
TROL_TBX are now available for use (along with the CESE solver) in TBX-based 
explosives simulations. 
•  Multi-nozzle injection mode is implemented for spray injection. 
•  Add logic to skip thermal computations during dynamic relaxation for a coupled 
thermal-structual problem (i.e.  when SOLN = 2 on the *CONTROL_SOLUTION 
keyword).  This does not affect the use of *LOAD_THERMAL keywords during 
dynamic relaxation. 
•  Implement  *DEFINE_CURVE_FUNCTION 
for  convection, 
flux,  radiation 
boundary 
•  conditions in thermal-only analyses, both 2D and 3D. 
•  *BOUNDARY_CONVECTION, *BOUNDARY_FLUX, and thermal dynamics are 
implemented for 20 node brick element. 
•  Include the reading of thermal data to *INCLUDE_BINARY. 
•  Allow *DEFINE_FUNCTION_TABULATED to be used in any place that requires 
a function of 1 variable.  Specifically, as a displacement scale factor with *INTER-
FACE_LINKING_NODE. 
•  Add  new  MUTABLE  option  for  *PARAMETER  and  *PARAMETER_EXPRES-
SION to indicate that it is OK to redefine a specific parameter even if *PARAME-
TER_DUPLICATION says redefinition is not allowed.  Also, only honor the first 
*PARAMETER_DUPLICATION card.
INTRODUCTION 
•  Add  functions  DELAY  and  PIDCTL  to  *DEFINE_CURVE_FUNCTION  for 
simulating PID (proportional-integral-derivative) controllers. 
•  *DEFINE_TABLE:  Add  check  of  table's  curves  for  mismatching  origin  or  end 
points. 
•  Update ANSYS library to version 16.0. 
•  Enhance report of "Elapsed time" in d3hsp. 
•  Add keyword *INCLUDE_UNITCELL to create a  keyword file containing user-
defined unit cell information with periodic boundary conditions. 
•  Add  *INCLUDE_AUTO_OFFSET:  the  node  and  element  IDs  of  the  include  file 
will  be  checked  against  IDs  of  the  previously  read  data  to  see  if  there  is  any 
duplication.  If duplicates are found, they will be replaced with another unique 
ID. 
Capabilities added to create LS-DYNA R9.0:  
See release notes (published separately) for further details. 
•  *AIRBAG 
◦  Disable  CPM  airbag  feature  during  DR  and  reactivate  in  the  transient 
phase. 
◦  *AIRBAG_WANG_NEFSKE_POP_ID pop venting based on RBIDP is now 
supported correctly (MPP only). 
◦  *AIRBAG_INTERACTION: 
  Fixed  MPP  airbag  data  sync  error  to  allow  final  pressure  among  in-
teracted airbags to reach equilibrium. 
◦  *AIRBAG_PARTICLE: 
  When  IAR = -1  and  Pbag  or  Pchamber  is  lower  than  Patm,  ambient 
air will inflate the bag through external vents and also fabric porosity. 
  Treat heat convection when chamber is defined. 
  Output pres+ and pres- to CPM interface forces file for internal parts. 
  Allow IAIR = 4 to gradually switch to IAIR = 2 to avoid instability. 
  Allow using shell to define inflator orifice.  The shell center and nor-
mal will be used as orifice node and flow vector direction. 
  Bug fix for porous leakage for internal fabric parts using CPM. 
  New feature to collect all ring vents into a single vent in order to cor-
rectly  treat  enhanced  venting  option.    All  the  vent  data  will  only  be 
output to the first part defined in the part set.
INTRODUCTION 
  Evaluate  airbag  volume  based  on  relative  position  to  avoid  trunca-
tion.    The  bag  volume  becomes  independent  of  coordinate  transfor-
mation. 
  Support  explicit/implicit  switch  and  dynamic  relaxation 
for 
*AIRBAG_PARTICLE. 
  Support vent/fabric blockage for CPM and ALE coupled analysis. 
  New option in *CONTROL_CPM to allow user defined smoothing of 
impact forces. 
  Fixed bug affecting *AIRBAG_PARTICLE_ID with PGP encryption. 
•  *ALE 
◦  *ALE_REFERENCE_SYSTEM_GROUP:  For  prtype = 4,  allow  the  ALE 
mesh to follow the center of mass of a set of nodes. 
◦  *CONTROL_ALE: 
  Add a variable DTMUFAC to control the time step related to the vis-
cosity from 
  *MAT_NULL (if zero, the viscosity does not control the time step). 
  Implement a 2D version of BFAC and CFAC smoothing algorithm. 
◦  *ALE_SMOOTHING:  Automatically  generate  the  list  of  3  nodes  for  the 
smoothing constraints and implement for MPP. 
◦  *SECTION_ALE2D,  *SECTION_SOLID_ALE:  Allow  a  local  smoothing 
controlled by AFAC,...,DFAC. 
◦  *ALE_SWITCH_MMG:  Allow  the  variables  to  be  modified  at  the  time  of 
the switch. 
◦  *CONTROL_REFINE_ALE:  Add  a  variable  to  delay  the  refinement  after 
removal  (DELAYRGN),  one  to  delay  the  removal  after  the  refinement 
(DELAYRMV), and one to prevent any removal in a certain radius around 
latest refinements (RADIUSRMV). 
◦  *ALE_STRUCTURED_MESH: Implemented structured ALE mesh solver to 
facilitate rectilinear mesh generation and to run faster. 
•  *BOUNDARY 
◦  *BOUNDARY_AMBIENT_EOS: 
Implement 
*DEFINE_CURVE_
FUNCTION for the internal energy and relative volume curves. 
◦  *BOUNDARY_AMBIENT: Apply ambient conditions to element sets. 
◦  Fix for adaptivity dropping SPCs in some cases (MPP only). 
◦  Added  conflict  error  checking  between  rigid  body  rotational  constraints 
(*CONSTRAINED_JOINT)  with 
joints  between 
rigid  bodies 
and 
*BOUNDARY_PRESCRIBED_ORIENTATION. 
◦  The first rigid body of the prescribed orientation cannot have any rotation-
al constraints.  Only spherical joints or translational motors can be used be-
tween the two rigid bodies of the prescribed orientation.  For now explicit
INTRODUCTION 
will be allowed to continue with these as warnings.Implicit will terminate 
at end of input checking. 
◦  Instead  of  error  terminating  with  warning  message,  STR+1371,  when 
*BOUNDARY_PRESCRIBED_MOTION  and  *BOUNDARY_SPC  are  ap-
plied  to  same  node  and  dof,  issue  warning  message,  KEY+1106,  and  re-
lease the conflicting SPC. 
◦  Fix  erroneous  results  if  *SET_BOX  option  is  used  for  *BOUNDARY_
PRESCRIBED_MOTION. 
◦  Fix  *BOUNDARY_PRESCRIBED_ACCELEROMETER_RIGID  for  MPP.    It 
may  error  terminate  or  give  wrong  results  if  more  than  one  of  this  key-
word are used. 
◦  Fix 
segmentation 
fault  when  using 
*BOUNDARY_PRESCRIBED_
ORIENTATION with vad = 2, i.e.  cubic spline interpolation. 
◦  Fix 
incorrect  behavior 
PLANE, i.e. > 1, are used. 
if  multiple  *BOUNDARY_SPC_SYMMETRY_
◦  Fix  incorrect  motion  if  *BOUNDARY_PRESCRIBED_MOTION_RIGID_
LOCAL is on a rigid part which is merged with a deformable part that has 
been switched to rigid using *DEFORMABLE_TO_RIGID. 
◦  Fix  incorrect  external  work  when  using  *BOUNDARY_PRESCRIBED_
MOTION with or without_RIGID option.  The dof specified in *BPM was 
not  considered  when  computing  the  external  work.    Also,  when  multiple 
*BPM  applied  to  the  same  node/rigid  body  with  different  dof  may  also 
cause incorrect computation of external work. 
incorrect  velocities  when  using 
*BOUNDARY_PRESCRIBED_
MOTION_RIGID_LOCAL  and  *INITIAL_VELOCITY_RIGID_BODY  for 
rigid bodies. 
◦  Fix 
◦  Implement  check  for  cases  where  *MAT_ACOUSTIC  nodes  are  merged 
with structural nodes on both sides of a plate element and direct the user 
to  the  proper  approach  to  this  situation  -  *BOUNDARY_ACOUSTIC_
COUPLING. 
◦  *BOUNDARY_ACOUSTIC_COUPLING  with  unmerged,  coincident  node 
coupling now implemented in MPP. 
◦  MPP 
logic 
corrected 
so 
*MAT_ACOUSTIC  and 
*BOUNDARY_
ACOUSTIC_COUPLING features may be used with 1 MPP processor. 
◦  Fixed  bug  for  *BOUNDARY_PRESCRIBED_MOTION  if  part  label  option 
is used. 
•  BLAST 
◦  Improve  *LOAD_BLAST_ENHANCED  used  with  ALEPID  option  in 
*LOAD_BLAST_SEGMENT: 
◦  Rearrange  the  ambient  element type  5  and  its  adjacent  element  into  same 
processor to avoid communications. 
◦  Eliminate several n-by-n searches for segment set and ambient type 5 with 
its neighboring elements to speed up the initialization.
INTRODUCTION 
◦  Change 
the  name  of  keyword  *DEFINE_PBLAST_GEOMETRY 
to 
*DEFINE_PBLAST_HEGEO. Both names will be recognized. 
•  *CESE (Compressible Flow Solver) 
◦  Modified  the  CESE  moving  mesh  CHT  interface  condition  calculation  to 
deal with some occasional MPP failures that could occur with mesh corner 
elements. 
◦  Improved  the  CESE  spatial  derivatives  approximation  in  order  to  bring 
better stability to the CESE solvers. 
◦  The 3D SMP and MPP CESE immersed boundary solvers now work with 
structural element erosion. 
◦  A new energy conservative conjugate heat transfer method has been added 
to the following 2D and 3D CESE Navier-Stokes equation solvers: 
  Fixed mesh (requires use of *CESE_BOUNDARY_CONJ_HEAT input 
cards) 
  Moving mesh FSI 
  Immersed boundary FSI 
◦  Prevent  the  fluid  thermal  calculation  from  using  too  short  a  distance  be-
tween the fluid and structure points in the new IBM CHT solvers. 
◦  In  the  under  resolved  situation,  prevent  the  CHT  interface  temperature 
from dipping below the local structural node temperature. 
◦  Add detection of blast wave arrival at CESE boundary condition face first 
sensing  the  leading  edge  of  the  pulse  (used  with  *LOAD_BLAST_
ENHANCED). 
◦  Set CESE state variable derivatives to more stable values for the blast wave 
boundary condition. 
◦  Corrected time step handling for the CESE Eulerian conjugate-heat transfer 
solver.  This affected only the reported output time. 
◦  Added CESE cyclic BC capability to the moving mesh CESE solver. 
◦  Fixed  some  issues  with  2D  CESE  solvers  where  the  mesh  is  created  via 
*MESH cards. 
◦  For the CESE solver coupled with the structural solver (FSI), corrected the 
time step handling. 
◦  For the CESE mesh motion solvers, and the ICFD implicit ball-vertex mesh 
motion solver, added a mechanism to check if all of the imposed boundary 
displacements  are  so  small  that  it  is  not  necessary  to  actually  invoke  the 
mesh  motion  solver.    This  is  determined  by  comparing  the  magnitude  of 
the imposed displacement at a node with the minimum distance to a virtu-
al ball vertex (that would appear in the ball-vertex method).  The relative 
scale  for  this  check  can  be  input  by  the  user  via  field  4  of  the  *CESE_
CONTROL_MESH_MOV card.
INTRODUCTION 
◦  Changed the NaN check capability for the CESE solvers to be activated on-
ly  upon  user  request.    This  is  input  via  a  non-zero  entry  in  field  7  of  the 
*CESE_CONTROL_SOLVER card. 
◦  Much like the ICFD solver, added a mechanism to adjust the distance used 
by the contact detection algorithm for the *CESE_BOUNDARY_FSI cards, 
as  well  as  the  new  moving  mesh  conjugate  heat  transfer  solvers.    This  is 
available through field 6 of the *CESE_CONTROL_SOLVER card. 
◦  Added a correction to the moving mesh CESE solver geometry calculation. 
◦  Corrected the initial time step calculation for both the 2D and 3D moving 
mesh CESE solvers. 
◦  For  the  moving  mesh  CESE  solver,  replaced  the  all-to-all  communication 
for fsi quantities with a sparse communication mechanism. 
•  *CHEMISTRY 
◦  The immersed boundary FSI method coupled with the chemistry solver is 
released. 
  Only Euler solvers, both in 2D and 3D, are completed with full chem-
istry. 
  Using this technique, CESE FSI Immerged Boundary Method coupled 
to  the  chemistry  solver  can  be  applied  to  high  speed  combustion 
problems such as explosion, detonation shock interacting with struc-
tures, and so on. 
  Some examples are available on our ftp site. 
•  *CONTACT 
◦  Fix MPP groupable contact problem that could in some cases have oriented 
the contact surfaces inconsistently. 
◦  Fix  bug  in  *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_TIED_
WELD. 
◦  Fix seg fault when using *CONTACT_AUTOMATIC_SINGLE_SURFACE_
TIED with consistency mode, .i.e.  ncpu < 0, for SMP. 
◦  Fix  false  warnings,  SOL+1253,  for  untied  nodes  using  *CONTACT_
AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK  and  *CONTACT_
AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE_TIEBREAK. 
◦  Fix  *CONTACT_TIED_SHELL_EDGE_TO_SURFACE  when  rigid  nodes 
are not tied even when ipback = 1.  This applies to SMP only. 
◦  Issue  warning if SOFT = 4 is used with an unsupported contact type, and 
reset it to 1. 
◦  Change  "Interface  Pressure"  report  in  intfor  file  from  abs(force/area)  to  -
force/area,  which  gives  the  proper  sign  in  case  of  a  tied  interface  in  ten-
sion.
INTRODUCTION 
◦  Increase  MPP  contact  release  condition  for  shell  nodes  that  contact  solid 
elements in SINGLE_SURFACE contact. 
◦  Fix for MPP IPBACK option for creating a backup penalty-based tied con-
tact. 
◦  Fix for MPP orthotropic friction in contact. 
◦  Fix for MPP *CONTACT_SLIDING_ONLY that was falsely detecting con-
tact in some cases. 
◦  Skip constraint based contacts when computing the stable contact time step 
size. 
◦  Add error trap if node set is input for slave side of single surface contact. 
◦  MPP:  some  fixes  for  constrained  tied  contact  when  used  with  adaptivity. 
The behavior of the slave nodes in adaptive constraints was not correct if 
they  were  also  master  nodes  of  a  tied interface.    This  has  been  fixed,  and 
support  for  the  rotations  required  for  CONTACT_SPOTWELD  have  also 
been added. 
◦  MPP:  update  to  AUTOMATIC_TIEBREAK  option  5  to  release  the  slave 
nodes (and report them as having failed) when the damage curve reaches 
0. 
◦  Fix made to routine that determines the contact interface segments, which 
was not handling pentahedral thick shell elements correctly. 
◦  MPP:  fix  for  strange  deadlock  that  could  happen  if  a  user  defines  a 
*CONTACT_FORCE_TRANSDUCER that has no elements in it and so gets 
deleted. 
◦  MPP contact: add support for *DEFINE_REGION to define an active con-
tact region. Contact occurring outside this region is ignored.  This  is only 
for MPP contact types: 
  AUTOMATIC_SINGLE_SURFACE 
  AUTOMATIC_NODES_TO_SURFACE 
  AUTOMATIC_SURFACE_TO_SURFACE 
  AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE 
◦  MPP fix for table based friction in non-groupable contact. 
◦  MPP:  add  frictional  work  calculation  for  beams 
in  *CONTACT_
AUTOMATIC_GENERAL. 
◦  Added new option "FTORQ" for contact.  Currently implemented only for 
beams in *CONTACT_AUTOMATIC_GENERAL in MPP.  Apply torque to 
the nodes to compensate for the torque introduced by friction.  Issue error 
message when users try to use SOFT = 2/DEPTH = 45 contact for solid el-
ements. 
◦  R-adaptivity,  ADPOPT = 7  in  *CONTROL_ADAPTIVE,  is  now  available 
for  SMP  version  of  *CONTACT_SURFACE_TO_SURFACE,_NODES_TO_
SURFACE,_AUTOMATIC_SURFACE_TO_SURFACE, 
and_
AUTOMATIC_NODES_TO_SURFACE (SOFT = 0 or 1 only).
INTRODUCTION 
◦  The  options  AUTOMATIC_SURFACE_TO_SURFACE_COMPOSITE  has 
been added to model composite processing.  The same option may be used 
to  model  certain  types  of  lubrication,  and  AUTOMATIC_SURFACE_TO_
SURFACE_LUBRICATION  may  be  used  instead  of  the  COMPOSITE  op-
tion for clarity.  (The two keyword commands are equivalent.) 
◦  Added  AUTOMATIC_SURFACE_TO_SURFACE_TIED_WELD  to  model 
the  simulation  of  welding.    As  regions  of  the  surfaces  are  heated  to  the 
welding temperature and come into contact, the nodes are tied. 
◦  Added 
*CONTACT_TIED_SHELL_EDGE_TO_SOLID. 
  This  contact 
transmits the shell moments into the solid elements by using forces unlike 
the SHELL_EDGE_TO_SURFACE contact with solid elements.  This capa-
bility  is  easier  for  users  than  *CONSTRAINED_SHELL_TO_SOLID.    The 
input is identical to *CONTACT_TIED_SHELL_EDGE_TO_SURFACE (ex-
cept for the keyword). 
◦  Fix incorrect motion of displayed rigidwall between 0.0 < time < birth_time 
when  birth  time > 0.0  for  *RIGIDWALL_GEOMETRIC_FLAT_MOTION_
DISPLAY.  The analysis was still correct.  Only the displayed motion of the 
rigidwall is incorrect. 
◦  Fix  corrupted 
intfor  when  using  parts/part  sets 
in  *CONTACT_
AUTOMATIC_.... This affects SMP only. 
◦  Fix  incorrect  stonewall  energy  when  using  *RIGIDWALL_PLANAR_
ORTHO. 
◦  Fix  unconstrained  nodes  when  using  *CONTACT_TIED_SURFACE_TO_
in  warning  message, 
SURFACE_CONSTRAINED_OFFSET  resulting 
SOL+540.  This affects SMP only. 
◦  Fix  spurious  repositioning  of  nodes  when  using  *CONTACT_SURFACE_
TO_SURFACE for SMP. 
◦  Enable  MAXPAR  from  optional  card  A  to  be  used  in  *CONTACT_TIED_
SURFACE_TO_SURFACE. It was originally hard-coded to 1.07. 
◦  The  shells  used  for  visualisation  of  *RIGIDWALL_PLANAR_MOVING_
DISPLAY  and  *RIGIDWALL_PLANAR_MOVING_DISPLAY  in  d3plot 
were not moving with the rigidwall.  This is now fixed. 
◦  Fix 
incorrect 
frictional 
forces 
if_ORTHO_FRICTION 
is  used 
in 
*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE. 
◦  Fix  seg  fault  when  using  *CONTACT_ENTITY  and  output  to  intfor  file 
with MPP, i.e.  s = intfor in command line. 
◦  Fix ineffective birth time for *CONTACT_TIED_NODES_TO_SURFACE. 
◦  Fix  untied  contacts  when  using  *CONTACT_TIED... 
  with  *MAT_
ANISOTROPIC_ELASTIC_PLASTIC/*MAT_157. 
◦  Fix MPP hang up when using *CONTACT_ENTITY. 
◦  Allow *CONTACT_AUTOMATIC_GENERAL to use MAXPAR from con-
tact  optional  card  A  instead  of  using  the  hard  coded  value  of  1.02.    This 
will better detect end to end contact of beams.  This applies to SMP only. 
◦  Fix  *CONTACT_TIED_SHELL_EDGE_TO_SURFACE  for  SMP  which  ig-
nores MAXPAR in contact optional card A.
INTRODUCTION 
◦  Fix seg fault when using *CONTACT_GUIDED_CABLE. 
◦  Fix  segmentation  fault  when  using  *CONTACT_AUTOMATIC_SINGLE_
SURFACE_TIED  in  consistency  mode,  i.e.    ncpu < 0  in  command  line,  for 
SMP. 
◦  Fix incorrect contacts when using *CONTACT_AUTOMATIC_GENERAL_
INTERIOR  for  beams  with  large  differences  in  thickness  and  when  the 
thinner  beams  are  closer  to  each  other than  to  the  thicker  beams.    Affects 
SMP only. 
◦  Fixed  force  transducers  with  MPP  segment  based  contact  when  segments 
are involved with multiple 2 surface force transducers.  The symptom was 
that  some  forces  were  missed  for  contact  between  segments  on  different 
partitions. 
◦  Fixed an MPP problem in segment based contact that cased a divide by ze-
ro during the bucket sort.  During an iteration of the bucket sort, all active 
segments were somehow in one plane which was far from the origin such 
that a dimension rounded to zero.  The fix for this should effect only this 
rare case and have no effect on most models. 
◦  Fixed thermal MPP segment based contact.  The message passing  of ther-
mal  energy  due  to  friction  was  being  skipped  unless  peak  force  data  was 
written to the intfor file. 
◦  Fixed  MPP  segment  based  implicit  contact.    A  flaw  in  data  handling 
caused possible memory errors during a line search. 
◦  Fixed implicit dynamic friction for segment based contact.  For sliding fric-
tion, the implicit stiffness was reduced to an infinitesimal value.  Also, the 
viscous  damping  coefficient  is  now  supported  for  implicit  dynamic  solu-
tions. 
◦  Fixed  segment  based  contact  when  the  data  has  all  deformable  parts  that 
are switched to rigid at the start of the calculation and then switched back 
to deformable prior to contact occurring.  A flaw was causing contact to be 
too soft.  This is now corrected. 
◦  Fixed a flaw  in  segment based  contact with  DEPTH = 25 that  could allow 
penetration to occur. 
◦  Improved  edge-to-edge  contact  checking  (DEPTH = 5,25,35)  and  the  slid-
ing  option  (SBOPT = 4,5)  in  areas  where  bricks  have  eroded  when  using 
segment based eroding contact. 
◦  Improved  the  initial  penetration  check  (IGNORE = 2  on  *CONTROL_
CONTACT) of segment based contact to eliminate false positives for shell 
segments.  Previously, the search was done using mid-plane nodes and the 
gap or penetration adjusted to account for segment thicknesses after.  The 
new way projects the nodes to the surface first and uses the projected sur-
face to measure penetration.  For brick segments with zero thickness there 
should  be  no  difference.    For  shell  segments,  the  improved  accuracy  will 
me more noticeable for thicker segments. 
◦  Improved  segment  based  contact  when  SHAREC = 1  to  run  faster  when 
there are rigid bodies in the contact interface.
INTRODUCTION 
◦  Fixed  a  possible  problem  during  initialization  of  segment  based  contact.  
Options  that  use  neighbor  segment  data  such  as  the  sliding  option  and 
edge-to-edge  checking  could  access  bad  data  if  the  same  nodes  were  part 
of both the slave and master surfaces.  This would not be a normal occur-
rence, but could happen. 
◦  Updated segment based contact to improve accuracy at points away from 
the origin.  The final calculations are now done with nodal and segment lo-
cations that have been shifted towards the origin so that coordinate values 
are small. 
◦  The  reporting  of  initial  penetrations  and  periodic  intersection  reports  by 
segment based contact was corrected for MPP solutions which were report-
ing incorrect element numbers. 
◦  Fixed memory errors in 2D automatic contact initialization when friction is 
used. 
◦  Fixed  2D  force  transducers  in  the  MPP  version  which  could  fail  to  report 
master surface forces.  Also fixed 2 surface 2D force transducers when the 
smp parallel consistency option is active. 
◦  Fixed 
*CONTACT_2D_AUTOMAITC_SINGLE_SURFACE  and  SUR-
FACE_TO_SURFACE which could exhibit unpredictable behavior such as 
a force spike or penetration. 
◦  Fixed  a  serious  MPP  error  in  the  sliding  option  of  *CONTACT_2D_
AUTOMATIC that could lead to error termination. 
◦  Fixed a problem with birth time for *CONTACT_2D_AUTOMATIC_TIED 
when used with sensor switching.  Also, fixed a problem in the contact en-
ergy calculation that could lead to abnormal terminations.  Finally, I made 
the process of searching for nodes to tie more robust as some problem was 
found with nodes being missed. 
◦  Fixed  a  2D  automatic  contact  bug  that  occurred  if  a  segment  had  zero 
length.    An  infinite  thickness  value  was  calculated  by  A/L  causing  the 
bucket sort to fail. 
◦  Added  support  for  *CONTACT_ADD_WEAR  for  smp  and  mpp  segment 
based (SOFT = 2) contact.  This option enables wear and sliding distance to 
be measured and output to the intfor file. 
◦  Added support to segment based contact for the SRNDE parameter on op-
tional card E of *CONTACT. 
◦  Added support to segment based eroding contact for SBOXID and MBOX-
ID on card 1 of *CONTACT. 
◦  Added support for *ELEMENT_SOURCE_SINK used with segment based 
contact.  With this update, inactive elements are no longer checked for con-
tact. 
◦  Added  a  segment  based  contact  option  to  allow  the  PSTIFF  option  on 
*CONTROL_CONTACT  to  be  specified  for individual  contact  definitions.  
The  new  parameter  is  PSTIFF  on  *CONTACT  on  optional  card  F,  field  1.  
Prior to this change, setting PSTIFF on *CONTROL_CONTACT set all con-
tact to use the alternate penalty stiffness method.  With this update, PSTIFF
INTRODUCTION 
on *CONTROL_CONTACT now sets a default value, and PSTIFF on card F 
can  be  used  to  override  the  default  value  for  an  individual  contact  inter-
face. 
◦  Added  support  for  REGION  option  on  optional  card  E  of  *CONTACT 
when using segment based, SOFT = 2 contact.  This works for all support-
ed keywords, SMP and MPP. 
◦  Added master side output in the MPP version for 2-surface force transduc-
ers when used with segment based (soft = 2) contact. 
◦  Added contact friction energy to the sleout database file for 
  _2D_AUTOMATIC_SURFACE_TO_SURFACE and 
  _2D_AUTOMATIC_SINGLE_SURFACE contact. 
◦  Enabled segment based contact (SMP and MPP) to work with type 24 (27-
node) solid elements. 
◦  Enabled  the  ICOR  parameter  on  *CONTACT,  optional  card  E  to  be  used 
with segment based (SOFT = 2) contact. 
◦  Fixed output to d3hsp for *CONTACT_DRAWBEAD using negative curve 
ID for LCIDRF 
◦  Add  slave  node  thickness  and  master  segment  thickness  as  input  argu-
ments to the *USER_INTERFACE_FRICTION subroutine usrfrc (SMP). 
◦  Forming mortar contact can now run with deformable solid tools and hon-
ors ADPENE to account for curvatures and penetrations in adaptive step.  
This applies to h- as well as r-adaptivity. 
◦  Single surface and surface-to-surface mortar contact accounts for rotational 
degrees  of  freedom  when  contact  with  beam  elements.    This  allows  for 
beams  to  "roll"  on  surfaces  and  prevents  spurious  friction  energy  to  be 
generated when in contact with rotating parts. 
◦  Maximum allowable penetration in forming and automatic mortar contacts 
is  hereforth  .5*(tslav+tmast)*factor  where  tmast = thickness  of  slave  seg-
ment and tmast = thickness of master segment.  The factor is hardwired to 
0.95, but is subject to change.  Prior to this it was .5*tslav, which seems in-
adequate (too small) in coping with initial penetrations in automotive ap-
plications using standard modeling approaches. 
◦  Up  to  now,  mortar  contact  has  only  acted  between  flat  surfaces,  now  ac-
count is taken for sharp edges in solid elements (the angle must initially be 
larger than 60 degrees), may have to increase the corresponding stiffness in 
the future. 
◦  When solid elements are involved in mortar contact the default stiffness is 
increased by a factor of 10.  This is based on feedback from customers indi-
cating that the contact behavior in those cases has in general been too soft.  
This may change the convergence characteristics in implicit but the results 
should be an improvement from earlier versions. 
◦  The  OPTT  parameter  on  *PART_CONTACT  for  the  contact  thickness  of 
beams is now supported in mortar contact.
INTRODUCTION 
◦  *CONTACT_ADD_WEAR: A wear law, Archard's or a user defined, can be 
associated with a contact interface to assess wear in contact.  By specifying 
WTYPE < 0  a  user  defined  wear  subroutine  must  be  written  to  customize 
the wear law.  For the Archard's wear law, parameters can depend on con-
tact pressure, relative sliding velocity and temperature.  Contacts support-
ed  are  *CONTACT_FORMING_SURFACE_TO_SURFACE,  *CONTACT_
FORMING_ONE_WAY_TO_SURFACE  and  *CONTACT_AUTOMATIC_
SURFACE_TO_SURFACE.    To  output  wear  data  set  NWEAR = 1  or 
NWEAR = 2  on  *DATABASE_EXTENT_INTFOR.    If  NWEAR  is  set  to  2 
then the sliding distance is output to the intfor file, in addition to the wear 
depth.  Otherwise only wear depth is output.  Also, the parameter NWUSR 
specifies the number of user wear history variables to be output in case a 
user defined wear routine is used.  By specifying CID (contact interface id) 
to a negative number, the wear depth will couple to the contact in the sim-
ulation in the sense that the penetration is reduced with wear.  The effect is 
that contact pressure will be redistributed accordingly but is only valid for 
relatively small wear  depths.  A  formulation for larger wear depths lie in 
the future which will require modification of the actual geometry. 
◦  Fixed bug affecting *CONTACT_RIGID_NODE_SURFACE (broken at rev.  
86847).  The bug was in reading *NODE_RIGID_SURFACE. 
◦  A bug fix in *CONTACT_DRAWBEAD_INITILIZE.  - The bug was caused 
by a sudden increase in effective strain after the element passed the draw-
bead.  When the increase in strain is too big, the search algorithm was not 
working reasonably in the material routine.  At the drawbead intersection 
point, an element could be initialized twice by  two bead curves, and cause 
abnormal thickness distribution. 
in 
*CONTACT_FORMING_ONE_WAY_SURFACE_TO_
SURFACE_SMOOTH  which  removes  the  limitation  that  the  contact  must 
be defined by segment set. 
◦  Fix  a  bug 
◦  SMOOTH option does not apply to FORMING_SURFACE_TO_SURFACE 
contact.  When the SMOOTH option is used, we now write a warning mes-
sage and disregard the SMOOTH option. 
•  *CONSTRAINED 
◦  *CONSTRAINED_LAGRANGE_IN_SOLID: 
Implement 
*CONSTRAINED_LAGRANGE_IN_SOLID_EDGE in 2D. 
◦  Fixed bug in *DAMPING_RELATIVE.  If the rigid part PIDRB is the slave 
part in *CONSTRAINED_RIGID_BODIES, the damping card did not work 
correctly.    There  is  a  work-around  for  previous  LS-DYNA  versions:  set 
PIDRB  to  the  master  part  in  *CONSTRAIEND_RIGID_BODIES,  not  the 
slave part. 
◦  *CONSTRAINED_RIGID_BODY_INSERT:  This  keyword  is  for  modeling 
die inserts.  One rigid body, called slave rigid body, is constrained to move
INTRODUCTION 
with another rigid body, called the master rigid body, in all directions ex-
cept for one. 
◦  A variety of enhancements for *CONSTRAINED_INTERPOLATION. 
  Enhanced  the  error  message  when  nodes  involved  in  the  constraint 
have been deleted. 
for 
row 
  Removed printing of 0 node ID in MPP. 
  Added a warning if there are too many (now set at 1000) nonzeroes in 
a  constraint 
*CONSTRAINED_INTERPOLATION  or 
*CONSTRAINED_LINEAR to protect implicit's constraint processing.  
These constraints will be processed differently in future releases.  We 
modified  the  constraint  processing  software  to  robustly  handle  con-
straint  rows  with  thousands  of  nonzero  entries.    We  added  error 
checking  for  co-linear  independent  nodes  as  these  constraints  allow 
singularities in the model. 
◦  Improved  implicit's  treatment  of  the  constraints  for  *CONSTRAINED_
BEAM_IN_SOLID. 
◦  Added error checking on the values of the gear ratios in *CONSTRAINED_
JOINTS. 
◦  *CONSTRAINED_BEAM_IN_SOLID: 
  Thick shell elements supported. 
  Wedge elements supported. 
  Debonding 
law  by  user-defined  subroutine  (set  variable  AX-
FOR > 1000). 
  Debonding law by *DEFINE_FUNCTION (set variable AXFOR < 0). 
◦  Error terminate with message, SOL+700, if CIDA and CIDB is not defined 
for *CONSTRAINED_JOINT_STIFFNESS_GENERALIZED. 
◦  Fix incorrect constraints on rotary dof for adaptivity. 
◦  Fix 
incorrect  motion 
in  *DEFORMABLE_TO_RIGID_
AUTOMATIC and if any of the *CONSTRAINED_NODAL_RIGID_BODY 
nodes belongs to a solid element. 
if  NRBF = 2 
◦  Fix input error when using large load curve ID for FMPH, FMT, FMPS in 
card  3  of  *CONSTRAINED_JOINT_STIFFNESS  with_GENERALIZED  or_
TRANSLATIONAL options. 
◦  Fix  seg  fault  if  using  tables  for  FMPH  of  *CONSTRAINED_JOINT_
STIFFNESS and if the angle of rotation is less than the the abscissa of the 
table or load curves. 
◦  Fixed an problem with *CONSTRAINED_BEAM_IN_SOLID when used in 
a model that also uses segment based eroding contact in the MPP version.  
This combination now works.
INTRODUCTION 
◦  Improved  the  precision  of  spot  weld  constraints  (*CONSTRAINED_
SPOTWELD) to prevent possible divide by zeroes when the inertia tensor 
is inverted.  This affects the single precision version only. 
◦  Fix 
for  damage 
SPOTWELD, MODEL = 2. 
function 
in 
*CONSTRAINED_INTERPOLATION_
◦  Add  some  user-friendly  output 
(rigid  body 
id) 
to  d3hsp 
for 
*CONSTRAINED_NODAL_RIGID_BODY_INERTIA. 
◦  Add  new  option  to  *CONSTRAINED_SPR2  to  connect  up  to  6  shell  ele-
ment  parts  (metal  sheets)  with  only  one  rivet  location  node.    This  is  in-
voked by defining extra part IDs for such a multi-sheet connection. 
◦  Add  more  flexibility  to  *CONSTRAINED_SPR2:  Load  curve  function  ex-
ponent  values  originally  hardwired  as  "8"  can  now  be  defined  with  new 
input parameters EXPN and EXPT. 
◦  Fixed  bug  wherein  the  joint  ID  in  *CONSTRAINED_JOINT_COOR  was 
read incorrectly. 
◦  Fixed  duplicate  ID  for  *CONSTRAINED_SPOTWELD,  ..._NODE_SET,_
POINTS and_SPR2. 
◦  Fix  keyword 
SPR4 
INTERPOLATION_SPOTWELD, where BETA2 was replaced by BETA3. 
◦  Significantly  reduce  the  memory  demand  in  the  initialization  stage  of 
*CONSTRAINED_
option 
reader 
for 
in 
*CONSTRAINED_MULTIPLE_GLOBAL for implicit analysis. 
◦  The  unit  cell  mesh  and  constraint  generated  by  *INCLUDE_UNITCELL 
now supports job ID. 
•  *CONTROL 
◦  Terminate  and  print  error  KEY+1117  for  cases  that  use  *INCLUDE_
TRANSFORM in 3d r-adaptvity.  More work is needed to make this com-
bination work. 
◦  Changed  SOL+41  message  ("reached  minimum  step")  from  an  error  to  a 
warning  and  terminate  normally.    This  message  is  triggered  when  the 
DTMIN criterion set in  *CONTROL_TERMINATION is reached. 
◦  Fixed  bug  in  which  h-adaptivity  missed  some  ADPFREQ-based  adapta-
tions when IREFLG < 0 (*CONTROL_ADAPTIVE). 
◦  Fixed  bug:  MS1ST  in  *CONTROL_TIMESTEP  causes  non-physical  large 
mass  and  inertia  on  Nodal  Rigid  Bodies  if  Dynamic  Relaxation  is  active.  
The error occurs at the start of the transient solution.  The mass can become 
very large, so the model may appear to be over-restrained. 
◦  Add new input check for curves.  After rediscretizing curves, check to see 
how well the original values can be reproduced.  If the match is poor, write 
out See variable CDETOL in *CONTROL_OUTPUT. 
◦  Added  the  ability  to  specify  unique  values  LCINT  for  each  curve,  which 
override the value set in *CONTROL_SOLUTION.  Note: the largest value 
of LCINT that appears will be used when allocating memory for each load
INTRODUCTION 
curve, so a single large value can cause significant increases in the memory 
required for solution. 
◦  The DELFR flag in *CONTROL_SHELL has new options for controlling the 
deletion of shell elements.  This feature is aimed at eliminating single, de-
tached elements and/or elements hanging on by one shared node. 
◦  Fix  spurious  deletion  of  elements  when  using  TSMIN.ne.0.0 
in 
*CONTROL_TERMINATION,  ERODE = 1  in  *CONTROL_TIMESTEP  and 
initialized implicitly in dynamic relaxation. 
◦  Fix spurious error, STR+755, if using *DAMPING_FREQUENCY_RANGE 
with *CONTROL_ADAPTIVE. 
◦  Add  new  feature  to  *CONTROL_SOLUTION,  LCACC,  to  truncate  load 
curve to 6 significant figures for single precision & 13 significant figures for 
double precision.  The truncation is done after applying the offset and scale 
factors. 
◦  Fix "*** termination due to mass increase ***' error when using mass scal-
ing with *ELEMENT_MASS_PART. 
◦  Fix  input  error  'node  set  for  nodal  rigid  body  #  not  found'  when  using 
*PART_INERTIA with *CONTROL_SUBCYCLE. 
◦  Fixed  the  negative  DT2MS  option  on  *CONTROL_TIMESTEP  for  thick 
shell types 5, 6, and 7. 
◦  Fixed bug in *CONTROL_CHECK_SHELL if PSID.lt.0 (part set ID) is used 
◦  Add  new  option  NORBIC  to  *CONTROL_RIGID  to  bypass  the  check  of 
rigid body inertia tensors being too small. 
◦  Add new option ICRQ to *CONTROL_SHELL for continuous treatment of 
thickness and plastic strain across element edges for shell element types 2, 
4, and 16 with max.  9 integration points through the thickness. 
◦  Add new option ICOHED to *CONTROL_SOLID.  If this value is set to 1, 
solid cohesive elements (ELFORM 19-22) will be eroded when neighboring 
(nodewise connected) shell or solid elements fail. 
◦  Beam  release  conditions  are  now  properly  supported  in  selective  mass 
scaling, see IMSCL on *CONTROL_TIMESTEP. 
◦  Modified MSGMAX in *CONTROL_OUPUT: MSGMAX  Maximum num-
ber of each error/warning message 
   > 0  number  of  message  to  screen  output,  all  messages  written  to 
messag/d3hsp 
   < 0 number of messages to screen output and message/d3hsp  
   = 0 the defaul is 50 
◦  Fix bugs in 3D solid adaptivity (*CONTROL_ADAPTIVE,ADPOPT = 7) so 
that the solid adaptivity will still work when there are any of the following 
in the model: 
  thick shells (*SECTION_TSHELL), 
  massless nodes,
INTRODUCTION 
  *LOAD_SEGMENT_{option}. 
◦  Added  PARA = 2  to  *CONTROL_PARALLEL  which  actives  consistent 
for 
force assembly in 
SMP.    An  efficient  parallel  algorithm  is  implemented  for  better  perfor-
mance when the consistency flag is turned on.  It shows better scaling with 
more cpus.  This option is overridden by parameter "para=" on the execu-
tion line. 
parallel 
•  DEM(Discrete Element Method) 
◦  Added output of following DES history variables to d3plot: 
  nodal stress and force 
  pressure 
  density 
  force chain 
  damage calculation when *DEFINE_DE_BOND is defined 
◦  Added  output  of 
following  DES  history  variables 
to  demtrh 
(*DATABASE_TRACER_DE): 
  coordination number 
  porosity and void ratio 
  stress 
  pressure 
  density 
◦  Output ASCII format for demrcf if BINARY.eq.3. 
◦  Implement  gauss  distribution  of  DE  sphere  radius  for  *DEFINE_DE_
INJECTION.  The mean radius is 0.5*(rmin+rmax) and standard deviation 
is 0.5*(rmax-rmin). 
◦  For  DE  sphere,  implement  the  stress  calculation  for  REV  (Representative 
Elementary  Volume)  using  *DATABASE_TRACER_DE  and  specific  RA-
DIUS. 
◦  Add  *BOUNDARY_DE_NON_REFLECTING  for  defining  non-reflecting 
boundary conditions for DE spheres. 
◦  For  *CONTROL_DISCRETE_ELEMENT,  add  the  option  to  create  the  liq-
uid  bridge  if  the  initial  distance  between  two  DE  spheres  is  smaller  than 
predefined gap. 
◦  Added  *DATABASE_DEMASSFLOW,  see  *DEFINE_DE_MASSFLOW_
PLANE,  for  measuring  the  mass  flow  of  DE  spheres  through  a  surface.  
The surface is defined by part or part set.  Output file is 'demflow'. 
◦  Add  *DEFINE_DE_INJECTION_ELLIPSE,  to  define  a  circular  or  elliptical 
injection plane.
INTRODUCTION 
◦  Add  *DEFINE_PBLAST_AIRGEO  for  *PARTICLE_BLAST  which  defines 
initial geometry for air particles. 
◦  Add DEM stress calculation when coupling with segment (*DEFINE_DE_
TO_SURFACE_COUPLING). 
◦  Fix error in demtrh file output (Window platform only). 
•  EFG (Element Free Galerkin) 
◦  Fix  bug  for  ELFORM = 41  implicit  when  there  are  6-noded/4-noded  ele-
ments. 
•  *ELEMENT 
◦  Fix a 2d seatbelt bug triggered by having both 1d and 2d  seatbelts, and a 
1d pretensioner of type 2, 3 or 9. 
◦  Fix MPP bug initializing multiscale spotweld in the unexpected case where 
the spotweld beam is merged with the shells rather than tied via contact. 
◦  Fix bug for *INCLUDE_UNITCELL. 
◦  *CONTROL_REFINE_...:  Implement  the  parent-children  transition  in 
*CONTACT_2D_SINGLE_SURFACE when a shell refinement occurs. 
◦  Fix error traps for *ELEMENT_SEATBELT_...  , for example, error termina-
tion due to convergence failure in retractors.  These error traps worked but 
could lead to a less graceful termination than other LS-DYNA error traps. 
◦  Correct calculation of wrap angle in seatbelt retractor. 
◦  Add MPP support for *ELEMENT_LANCING. 
◦  *ELEMENT_SEATBELT: 
  Fix  a  MPP  belt  bug  that  can  happen  when  buckle  pretensioner  is 
modeled as a type-9 pretensioner. 
  2D belt and 1D belt now can share the same *MAT_SEATBELT. 
  The  section  force  for  2d  belt  is  recoded  to  provide  more  robust  and 
accurate     results. 
  The loading curve LLCID of *MAT_SEATBELT can  be a table defin-
ing strain-rate dependent stiffness curve. 
  IGRAV  of  *ELEMENT_SEATBELT_ACCELEROMETER  can  be  a 
curve defining gravitation flag as a function of time. 
◦  Add *NODE_THICKNESS to override shell nodal thickness otherwise de-
termined  via  *SECTION_SHELL,  *PART_COMPOSITE,  or  *ELEMENT_
SHELL_THICKNESS. 
◦  Fix input error when using *DEFINE_ELEMENT_DEATH with BOXID > 0 
for MPP. 
◦  Implement subcycling for thick shells. 
◦  Fix  ineffective  *DEFINE_HAZ_PROPERTIES  when  solid  spotwelds  and 
hex spotweld assemblies are both present.
INTRODUCTION 
◦  Fix incorrect beta written out for *ELEMENT_SHELL_BETA in dynain file 
when *PART_COMPOSITE keyword is present in the original input. 
◦  Fix  NaN  output  to  elout_det  and  spurious  element  deletion  if  NO-
DOUT = STRAIN or STRAIN_GL or ALL or ALL_GL. 
◦  Fix  incorrect  reading  of  TIME  in  card  3  of  *ELEMENT_SEATBELT_
SENSOR SBSTYP = 3 when long = s in command line. 
◦  *PART_COMPOSITE:  Increased  the  explicit  solution  time  step  for  thin 
shell  composite  elements.    The  existing  method  was  overly  conservative.  
The new method is based on average layer stiffness and density. 
◦  In  conjunction  with  the  above  change  in  composite  time  step  calculation, 
increase  nodal  inertia  in  the  rare  cases  of  *PART_COMPOSITE  in  which 
the  bending  stability  is  not  satisfied  by  the  membrane  stability  criterion.  
The  inertia  is  only  increased  in  the  cases  where  it  is  necessary;  for  most 
models this change has no effect, but this can occur in the case of sandwich 
sections with stiffer skins around a less stiff core. 
◦  Corrected rotational inertia of thin shells when layers have mixed density 
and the outer layers are more dense than inner layers.  The fix will mostly 
affect elements that are very thick relative to edge length. 
◦  Fixed  default  hourglass  control  when  the  *HOURGLASS  control  card  is 
used but no HG type is specified.  We were setting to type 1 instead of 2.  
Also,  fixed  the  default  HG  types  to  match  the  User's  Manual  for  implicit 
and explicit. 
◦  Fixed the part mass that was reported to d3hsp when *ELEMENT_SHELL_
SOURCE_SINK is used.  The inactive elements were being included caus-
ing too high mass. 
◦  Prevent  inactive  shell  elements  (from  *ELEMENT_SHELL_SOURCE_
SINK) from controlling the solution time step. 
◦  Fixed  the  reported  strain  tensor  in  elements  created  by  *ELEMENT_
SHELL_SOURCE_SINK when strain output is requested.  The history was 
being retained from the previous elements with the same ID. 
◦  Fixed  torsion  in  linear  beam  form  13.    A  failure  to  add  the  torsional  mo-
ment  at  node  2  caused  an  inability  to  reach  equilibrium  in  the  torsional 
mode. 
◦  Fixed  solid  element  4  so  that  rigid  body  translation  will  not  cause  strain 
and stress due to round-off error. 
◦  Mixed parallel consistency when used with solid element type 20.  A buffer 
was not being allocated leading to a memory error. 
◦  Changed  the  MPP  behavior  of  discrete  beams  (ELFORM = 6)  when  at-
tached  to  elements  that  fail.    They  were  behaving  like  null  beams,  in  the 
sense that it was possible for beam nodes to become dead due to attached 
elements failing, and discrete beams would be no longer visualized even if 
the beams themselves had not failed.  With this change, the MPP discrete 
beams  now  behave  like  other  beams  in  that the  beams  have  to  fail  before 
they are removed.  MPP and SMP behavior is now consistent.
INTRODUCTION 
◦  Improved the precision of the type 2 Belytschko Schwer resultant beam to 
prevent energy growth in single precision. 
◦  Fixed  the  NLOC  option  on  *SECTION_SHELL  for  the  BCIZ  triangle  ele-
ments (ELFORM = 3) and the DKT triangle elements (ELFORM = 17).  The 
offset was scaled by the solution time step so typically the offset was much 
smaller than expected. 
◦  Fixed elout stress output for shell element forms 23 and 24.  The in-plane 
averaging was incorrect causing wrong output. 
◦  Changed  *ELEMENT_TSHELL  so  that  both  the  COMPOSITE  and  BETA 
options  can  be  read  at  the  same  time.    Prior  to  the  fix,  only  the  first  one 
would be read. 
◦  Fixed all thick shells to work with anisotropic thermal strains which can be 
defined  by  *MAT_ADD_THERMAL.    Also,  this  now  works  by  layer  for 
layered composites. 
◦  Fixed  implicit  solutions  with  thick  shells  with  *MAT_057  when  there  are 
also solid elements in the model that use *MAT_057.  Thick shells support 
only the incremental update of the F tensor but a flag was set incorrectly in 
the material model. 
◦  Fixed *MAT_219 when used with thick shell types 3, 5, and 7.  A failure to 
initialize terms for the time step caused a possible wrong time step. 
◦  Fixed  orthotropic  user  defined  materials  when  used  with  thick  shell  ele-
ments.  The storing of the transformation matrix was in the wrong location 
leading to wrong stress and strain. 
◦  For thick shell composites that use element forms 5 and 7, the user can now 
use  laminated  shell  theory  along  with  the  TSHEAR = 1  on  *SECTION_
TSHELL to get a constant shear stress through the thickness with a compo-
site. 
◦  Fixed  the  initialization  of  *MAT_CODAM2/*MAT_219  when  used  with 
thick shell forms 3, 5, or 7.  The 3D thick shell routine uses only 2 terms for 
the  transformation  and  therefore  needs  unique  initialization  of  the  trans-
formation data. 
◦  Fixed  thick  shell  types  3  and  5    when  used  in  implicit  solutions  with 
*MATs  2,  21,  261,  and  263.    The  material  constitutive  matrix  for  *MATs  2 
and  21  was  not  rotated  correctly  causing  wrong  element  stiffness.    The 
constitutive matrix for *MATs 261 and 263 was not orthotropic.  Also, for 
*MAT_021,  type  5  thick  shell  needed  some  material  terms  defined  to  cor-
rect the assumed strain. 
◦  Fixed thick shell forms 3 and 5 when used in implicit solutions with non-
isotropic materials.  The stiffness matrix was wrong due to incorrect trans-
formations. 
◦  Also,  fixed  the  implicit  stiffness  of  thin  and  thick  shells  when  used  with 
laminated  shell 
(LAMSHT = 3,4,5  on 
*CONTROL_ACCURACY).    Elements  were  either  failing  to  converge  or 
converging more slowly due to the failure to adjust the stiffness matrix to 
be consistent with the assumed strain. 
theory  by  assumed  strain
INTRODUCTION 
◦  Added  support  for  *ELEMENT_SHELL_SOURCE_SINK  to  form  2  ele-
ments with BWC = 1 on *CONTROL_SHELL. 
◦  Fixed the s-axis and t-axis orientation of beam spot welds in the MPP ver-
sion when those beam weld elements are defined with a 3rd node.  The 3rd 
node was being discarded prior to initializing the beam orientation so the s 
and t-axes were being randomly assigned as if the 3rd node had not been 
assigned.  The effect on solutions is likely fairly minimal since beam mate-
rial is isotropic and failure typically is too, but may not be. 
◦  Added Rayleigh damping (*DAMPING_PART_STIFFNESS) for thick shell 
formulations  1,  2,  and  6.    Previously,  it  was  available  for  only  the  thick 
shells that call 3D stress updates, (forms 3 and 5), but now it is available for 
all thick shell formulations. 
◦  Added  new  SCOOR  options  for  discrete  beam  section  6  (*SECTION_
BEAM).    A  flaw  was  found  in  how  the  discrete  beam  accounts  for  rigid 
body  rotation  when  SCOOR = -3,  -2,  +2,  and  +3.    A  correction  for  this  is 
made and introduced as new options, SCOOR = -13, -12, +12, and +13.  A 
decision was made to leave the existing options SCOOR = -2, +2, -3 and +3 
unchanged so that legacy data could run without changes. 
◦  Enabled  the  ELFORM  18  linear  DKT  shell  element  to  work  with  *PART_
COMPOSITE  and  with  an  arbitrary  number  of  through  thickness  integra-
tion points.  It was limited to a single material and 10 Gauss points. 
◦  Added  the  possibility  to  write  *ELEMENT_SOLID_ORTHO  into  dynain 
file  if  requested.    To  activate  this  add  OPTCARD  to  *INTERFACE_
SPRINGBACK and set SLDO = 1. 
◦  Refine  characteristic  length  calculation  for  27-node  solid  (ELFORM  24).  
This change may increase the time step substantially for badly distorted el-
ements. 
◦  Implement selective reduced integration for 27-node solid (ELFORM 24). 
◦  Allow  part  sets  to  be  used  in  *DEFORMABLE_TO_RIGID_AUTOMATIC.  
Either  PID  is  defined  negative  or  "PSET"  is  set  in  column  3  (D2R)  or  2 
(R2D). 
◦  Add new option STRESS = 2 to *INCLUDE_STAMPED_PART: no stresses 
and no history variables are mapped with that setting. 
◦  New  keyword  *PART_STACKED_ELEMENTS  provides  a  method  to  de-
fine and to discretize layered shell-like structures by an arbitrary sequence 
of shell and/or solid elements over the thickness. 
◦  The geometric stiffness matrix for the Belytschko beam element type 2 has 
been  extended  to  include  nonsymmetric  terms  arising  from  nonzero  mo-
ments.  Provides "almost" quadratic convergence, still some terms missing 
to  be  added  in  the  future.    Also  support  a  strongly  objective version  acti-
vated by IACC on *CONTROL_ACCURACY. 
◦  The geometric stiffness for the Hughes-Liu element type 1 is fixed. 
◦  Fix parsing error in *SECTION_BEAM_AISC.
•  EM (Electromagnetic Solver) 
INTRODUCTION 
◦  Add the new EM 2d axi solver in SMP and MPP for EM solver 1 (eddy cur-
rent).  It is coupled with the mechanics and thermal solvers. 
◦  The new EM 2d can be used with RLC circuits on helix/spiral geometries 
using *EM_CIRCUIT_CONNECT. 
◦  Add EM contact into new EM 2d axi, in SMP and MPP. 
◦  Add *EM_BOUNDARY support in new EM 2d axi solver. 
◦  Introduce scalar potential in new EM 2d axi.  The 2d axi can also  be cou-
pled with imposed voltage. 
◦  Add new keyword *EM_CIRCUIT_CONNECT to impose linear constraints 
between circuits with imposed currents in 3d solvers.  This allows for ex-
ample to impose that the current in circuit 1 is equal to the current in cir-
cuit 2 even if the 2 corresponding parts are not physically connected. 
◦  Add *EM_VOLTAGE_DROP keyword to define a voltage drop between 2 
segment  sets.    This  voltage  drop  constraint  is  coupled  to  the  contact  con-
straint  so  that  the  contact  (voltage  drop = 0)  has  priority  over  the  *EM_
VOLTAGE_DROP constraint. 
◦  Add *EM_CONTROL_SWITCH_CONTACT keyword to turn the EM con-
tact detection on and off. 
◦  NCYCLBEM/NCYCLFEM in *EM_SOLVER_...  can now be different than 
1 when EM_CONTACT detected. 
◦  Add RLC circuit for type 3 solver (resistive heating). 
◦  Add  computation  of  mutuals/inductances  in  2d  axi  for  output  to  em_
circuit.dat 
◦  Add  criteria  on  autotimestep  calculation  when  R,L,C  circuit  used  to  take 
into account R,L,C period. 
◦  Fix keyword counter in d3hsp. 
◦  Better and clearer output to terminal screen. 
◦  Support jobid for EM ascii file outputs. 
•  Forming 
◦  Improvements to trimming: 
  *DEFINE_CURVE_TRIM_NEW: if trim seed node is not defined, we 
will search a seed node based on nodes from the sheet blank and the 
inside/outside flag definition for the trimming curves. 
  Map strain tensors to triangular elements after trimming. 
◦  Add a new function to the trim of solid elements in normal (3-D) trimming 
case,  related  to  *DEFINE_CURVE_TRIM_3D.    If  the  trimming  curve  is 
close to the bottom side, set TDIR = -1.  If the trimming curve is close to the  
upper side, set TDIR = 1.
INTRODUCTION 
◦  Add to *ELEMENT_LANCING.  Allow parametric expression for variables 
END and NTIMES. 
◦  A  bug  fix  for  *CONTROL_FORMING_AUTOPOSITION_PARAMETER_
SET: Fix distance calculation error when the target mesh is too coarse. 
◦  Improvements to springback compensations: 
  Output  the  new  trimming  curve  with  *DEFINE_CURVE_TRIM_3D 
(previously  *DEFINE_CURVE_TRIM),  so  that  it  can  be  easily  con-
verted to IGES curve by LS-PrePost.  or used in another trimming cal-
culation. 
  Output  each  curve  to  IGES  format  in  the  following  name  format: 
newcurve_scp001.igs,  newcurve_scp002.igs,  newcurve_scp003.igs, 
etc. 
  Output  change  in  file  "geocur.trm".    This  update  will  allow  change 
from  *DEFINE_CURVE_TRIM(_3D,_NEW),  whatever  is  used  for  in-
put. 
◦  Add  a  new  keyword:  *DEFINE_FORMING_CONTACT  to  facilitate  the 
forming contact definitions. 
◦  Add a new keyword *DEFINE_FORMING_CLAMP, to facilitate clamping 
simulation. 
◦  A  new  feature  in  mesh  fusion,  which  allows  a  moving  box  to  control  the 
fusion, only if the center of the elements is inside the box can the elements 
can  be  coarsened.    Can  be  used  in  conjuntion  with  *DEFINE_BOX_
ADAPTIVE. 
◦  Add a new feature to *DEFINE_BOX_ADAPTIVE: Moving box in adaptiv-
ity, useful in roller hemming and incremental forming. 
◦  In mesh coarsening, if the node is defined in a node set, the connected ele-
ments  will  be  kept  from  being  coarsened.    Previously, only  *SET_NODE_
LIST was supported.  Now option *SET_NODE_GENERAL is allowed. 
◦  Add a new function: mesh refinement for sandwich part.  The top and bot-
tom  layers  are  shell  elements  and  the  middle  layer  is  solid  elements.    Set 
IFSAND to 1 in *CONTROL_ADAPTIVE. 
  Applies to both 8-noded and 6-noded solid elements. 
  Map stress and history variables to the new elements. 
◦  New 
features  related 
BLANKSIZE_DEVELOPMENT: 
to  blank  size  development  *INTERFACE_
  Add  *INTERFACE_BLANKSIZE_SYMMETRIC_PLANE  to  define 
symmetric plane in blank size development 
  Add  *INTERFACE_BLANKSIZE_SCALE_FACTOR.    For  each  trim-
ming, different scale factors can be used to compensate the blanksize.  
This is especially useful when the inner holes are small.  Includes an
INTRODUCTION 
option  of  offset  the  target  curve  which  is  useful  if  multiple  target 
curves (e.g., holes) and formed curves are far from each other. 
  Allow target curve to be outside of the surface of the blank. 
  Add sorting to the mesh so the initial mesh and the formed mesh do 
not need to have the same sequence for the nodes. 
  Add a new variable ORIENT, set to "1" to activate the new algorithm 
to  potentially  reduce  the  number  of  iterations  with  the  use  of 
*INTERFACE_BLANKSIZE_SCALE_FACTOR (scale = 0.75 to 0.9). 
  Fix smooth problem along calculated outer boundary. 
  Automatically determine the curve running directions (IOPTION = 2 
and -2 now both give the same results). 
  Accept parameteric expression. 
◦  A  bug  fix  for  springback  compensation:  *INCLUDE_COMPENSATION_
SYMMETRIC_LINES  Fix  reading  problem  of  free  format  in  the  original 
coding. 
◦  Add  a  new  keyword  *CONTROL_FORMING_BESTFIT.    Purpose:    This 
keyword  rigidly  moves  two  parts  so  that  they  maximally  coincide.    This 
feature can be used in sheet metal forming to translate and rotate a spring 
back  part  (source)  to  a  scanned  part  (target) to  assess  spring  back  predic-
tion accuracy.  This keyword applies to shell elements only. 
◦  Improvements to *CONTROL_FORMING_AUTOCHECK: 
  When  IOFFSET = 1,  rigid  body  thickness  is  automatically  offset, 
based  on  the  MST  value  defined  in  *CONTACT_FORMING_ONE_
WAY_SURFACE. 
  Add new variable IOUTPUT that when set to 1 will output the offset 
rigid tool mesh, and the new output tool file is: rigid_offset.inc.  After 
output the simulation stops.  See R9.0 Manual for further details. 
  When  both  normal  check  and  offset  are  used,  small  radius  might 
cause  problem  for  offsetting.    The  new  modification  will  check  the 
normal again after offsetting the tool 
  When outputting the rigid body mesh, output the bead nodes also. 
  Changes  to  *CONTROL_FORMING_AUTOCHECK  when  used  to-
gether with SMOOTH option: check and fix rigid body bad elements 
before converting the master part ID to segment set id to be used by 
SMOOTH option. 
  Set IOUTPUT.eq.  3 to output rigid body mesh before and after offset. 
  Fix problems offseting a small radius to a even smaller radius. 
  Remove T-intersection. 
◦  For *CONTROL_IMPLICIT_FORMING, fix output messages in d3hsp that 
incorrectly  identified  steps  as  implicit  dynamic  when  they  were  actually 
implicit static. 
◦  Improve *CONTROL_FORMING_UNFLANGING:
INTRODUCTION 
  Automatically calculate CHARLEN, so user does not need to input it 
anymore. 
  Allow nonsmooth flange edge. 
  Instead  of  using  preset  value  of  0.4  (which  works  fine  for  thin  sheet 
metal), blank thickness is now used to offset the slave node (flanges) 
from the rigid body (die). 
•  *FREQUENCY_DOMAIN 
◦  *FREQUENCY_DOMAIN_RANDOM_VIBRATION: Fixed a bug in dump-
ing d3psd binary database, when both stress and strain are included. 
◦  *FREQUENCY_DOMAIN_SSD_ERP: Implemented the Equivalent adiated 
Power (ERP) computation to MPP. 
◦  *FREQUENCY_DOMAIN_ACOUSTIC_BEM: 
  Enabled  running  dual  collocation  BEM  based  on  Burton-Miller  for-
mulation  (METHOD = 4)  with  vibration  boundary  conditions  pro-
vided  by  Steady State Dynamic  analysis  (*FREQUENCY_DOMAIN_
SSD). 
  Added exponential window function for FFT (FFTWIN = 5). 
  Implemented a new forward and backward mixed radix FFT. 
  Implemented  acoustic  computation  restart  from  frequency  domain 
boundary  conditions,  in  addition  to  time  domain  boundary  condi-
tions (RESTRT = 1). 
  Enabled  out-of-core  velocity  data  storage,  to  solve  large  scale  prob-
lems. 
  Implemented  option  HALF_SPACE  to  Rayleigh  method  (METH-
OD = 0) to consider acoustic wave reflection. 
  Added  velocity  interpolation  to  take  care  of  mismatching  between 
acoustic  mesh  and  structural  mesh  (*BOUNDARY_ACOUSTIC_
MAPPING),  for  the  case  that  the  boundary  conditions  are  provided 
by Steady State Dynamic analysis. 
  Added weighted SPL output to acoustic computation (DBA = 1,2,3,4). 
  Implemented radiated sound power, and radiation efficiency compu-
tation  to  collocation  BEMs  (METHOD = 3,4).    Added  new  ASCII  xy-
plot databases Press_Power and Press_radef to save the sound power 
and radiation efficiency results. 
  Enabled  using  both  impedance  and  vibration  (velocity)  boundary 
conditions in acoustic simulation. 
◦  *FREQUENCY_DOMAIN_ACOUSTIC_FEM: 
  Added weighted SPL output to FEM acoustics (DBA = 1,2,3,4). 
  Implemented  option  EIGENVALUE  to  perform  acoustic  eigenvalue 
analysis; added ASCII database eigout_ac to save acoustic eigenvalue
INTRODUCTION 
results; added binary plot database d3eigv_ac to save acoustic eigen-
vectors. 
  Enabled  consideration  of  nodal  constraints  in  acoustic  eigenvalue 
analysis. 
  Enabled  FEM  acoustic  analysis  with  frequency  dependent  complex 
sound speed. 
  Implemented pressure and impedance boundary conditions. 
◦  *FREQUENCY_DOMAIN_ACOUSTIC_FRINGE_PLOT: 
  Added this keyword to 1) generate acoustic field points as a sphere or 
plate mesh (options SPHERE and PLATE), or 2) define acoustic field 
points mesh based on existing structure components (options PART, 
PART_SET and NODE_SET) so that user can get fringe plot of acous-
tic  pressure  and  SPL.    The  results  are  saved  in  binary  plot  database 
d3acs  (activated  by  keyword  *DATABASE_FREQUENCY_BINARY_
D3ACS). 
◦  *FREQUENCY_DOMAIN_RANDOM_VIBRATION: 
  Changed  displacement  rms  output  in  d3rms  to  be  the  displacement 
itself, without adding the original nodal coordinates. 
  Implemented von mises stress PSD computation in beam elements. 
  Implemented fatigue analysis with beam elements. 
  Added strain output to binary plot databases d3psd and d3rms, and 
binout database elout_psd. 
  Added initial damage ratio from multiple loading cases (INFTG > 1). 
◦  *FREQUENCY_DOMAIN_SSD: 
  Implemented option ERP to compute Equivalent Radiated Power.  It 
is  a  fast  and  simplified  way  to  characterize  acoustic  behavior  of  vi-
brating  structures.  The  results  are  saved  in  binary  plot  database 
d3erp  (activated  by  keyword  *DATABASE_FREQUENCY_BINARY_
D3ERP), and ASCII xyplot files ERP_abs and ERP_dB. 
  Implemented  fatigue  analysis  based  on  maximum  principal  stress 
and maximum shear stress. 
•  ICFD (Incompressible Flow Solver) 
◦  *ICFD_BOUNDARY_FSWAVE:  Added  a  boundary  condition  for  wave 
generation of 1st order stokes waves with free surfaces. 
◦  *ICFD_DATABASE_DRAG_VOL:  For  computing  pressure  forces  on  vol-
umes  ID  (useful  for  forces  in  porous  domains),  output  in  icfdragivol.dat 
and icfdragivol.#VID.dat.
INTRODUCTION 
◦  *ICFD_CONTROL_DEM_COUPLING:  Coupling  the  ICFD  solver  with 
DEM particles is now possible. 
◦  *ICFD_CONTROL_MONOLITHIC: Added a monolithic solver (=1) which 
can be selected instead of the traditional fractional step solver (=0). 
◦  *ICFD_CONTROL_POROUS:  This  keyword allows  the  user  to  choose  be-
tween the Anisotropic Generalized Navier-Stokes model (=0) or the Aniso-
tropic  Darcy-Forchheimer  model  (=1)  (for  Low  Reynolds  number  flows).  
The Monolithic solver is used by default for those creeping flows. 
◦  *ICFD_CONTROL_TURBULENCE: 
  Modified existing standard k-epsilon. 
  Added Realizable k-epsilon turbulence model. 
  Added  Standard  98  and  06  Wilcox  and  Menter  SST  03  turbulence 
models. 
  Added Several laws of the wall. 
  Added Rugosity law when RANS turbulence model selected. 
◦  *ICFD_MODEL_POROUS: 
  Added Porous model 5 for anistropic materials defined by P-V exper-
imental curves. 
  Added  porous  model  6  for  moving  domain  capabilities  for  Porous 
Media volumes using load curves for permeabilities directions. 
  Added  porous  model  7  for  moving  domain  capabilities  for  Porous 
Media  volumes  using  ICFD_DEFINE_POINT  for  permeabilities  di-
rections. 
  Added  porous  model  9  for  a  new  Anisotropic  Porous  Media  flow 
model (PM model ID = 9): It uses a variable permeability tensor field 
which is the result of solid dynamic problems.  The model reads the 
solid  mesh  and  the  field  state  and  maps  elemental  permeability ten-
sor and solid displacements to the fluid mesh. 
◦  *ICFD_MODEL_NONNEWT: 
  Added  a  few  models  for  non  newtonian  materials  and  temperature 
dependant viscosity : 
•  model 1 : power law non newtonian (now also temperature 
dependant) 
•  model 2 : carreau fluid 
•  model 3 : cross fluid 
•  model 4 : herschel-bulkley 
•  model 5 : cross fluid II 
•  model 6 : temperature dependant visc (sutherland) 
•  model 7 : temperature dependant visc (power law)
INTRODUCTION 
•  model  8  :  load  curve  dependant  visc,  model  8  is  especially 
interesting since a DEFINE_FUNCTION can be used (for so-
lidification applications). 
◦  *ICFD_SOLVER_TOL_MONOLITHIC:  Used  to  define  atol,  rtol,  dtol  and 
maxits  linear  solver  convergence  controls  of  the  monolithic  NS  time  inte-
gration 
◦  *MESH_BL: Added  support for boundary layer mesh creation by  specify-
ing  the  thickness,  number  of  layers,  first  node  near  the  surface  and  the 
strategy to use to divide and separate the elements inside the BL adding. 
◦  *ICFD_BOUNDARY_PRESCRIBED_VEL: Added  the  support  of  DEFINE_
FUNCTION making the second line of the keyword obsolete. 
◦  *ICFD_CONTROL_TIME: Min and Max timestep values can be set. 
◦  *ICFD_DATABASE_DRAG: 
  Added frequency output. 
  Added option to output drag repartition percentage in the d3plots as 
a surface variable. 
◦  *ICFD_CONTROL_IMPOSED_MOVE:  This  keyword  now  uses  *ICFD_
PART  and  *ICFD_PART_VOL  instead  of  *MESH_VOL  for  ID.    It  is  now 
possible to impose a rotation on a part using Euler angles. 
◦  *ICFD_CONTROL_OUTPUT: 
  Field 4 now to output mesh in LSPP format and in format to be run 
by the icfd solver (icfd_fluidmesh.key and icfd_mesh.key) 
  icfd_mesh.key  now  divides  the  mesh  in  ten  parts,  from  best  quality 
element decile to worst. 
  A new mesh is now output at every remeshing. 
  Added support for parallel I/O for Paraview using the PVTU format. 
◦  *ICFD_DEFINE_POINT: Points can now be made to rotate or translate. 
◦  *ICFD_MAT: 
  Nonnewtonian models and Porous media models are now selected in 
the third line by using the new ICFD_MODEL keyword family. 
  HC and TC can now be made temperature dependent. 
◦  *ICFD_CONTROL_DIVCLEAN:  Added  option  2  to  use  a  potential  flow 
solver to initialize the Navier Stokes solver. 
◦  *ICFD_CONTROL_FSI:  Field  5  provides  a  relaxation  that  starts  after  the 
birthtime. 
◦  *ICFD_CONTROL_MESH:  Field  3  added  a  new  strategy  to  interpolate  a 
mesh size during the node insertion.  In some cases it speeds up the mesh-
ing  process  and  produces    less  elements.    Field  4  changes  the  meshing 
strategy in 2d.
INTRODUCTION 
◦  *ICFD_CONTROL_SURFMESH:  Added 
meshing/adaptation of surface meshing. 
support 
for  dynamic 
re-
◦  *ICFD_BOUNDARY_PRESCRIBED_VEL:VAD = 3  now  works  with 
DOF = 4. 
◦  SF can be lower than 0. 
◦  PID can be over 9999 in *ICFD_DATABASE_FLUX. 
◦  Fixed d3hsp keyword counter. 
◦  Clarified terminal output. 
◦  Y+ and Shear now always output on walls rather than when a turbulence 
model was selected. 
◦  Added  coordinate  of  distorted  element  before  remeshing  occurs.    Output 
on terminal and messag file 
◦  Fixed bug in conjugate heat transfer cases.  When an autotimestep was se-
lected in *ICFD_CONTROL_TIME, it would always only take the thermal 
timestep. 
◦  An estimation of the CFL number is now output in the d3plot files.  This is 
not the value used for the autotimestep calculation. 
◦  Turbulence intensity is now output in the d3plots. 
◦  Jobid now supported for ICFD ASCII File outputs. 
◦  Fixed communication of turbulent constants in MPP. 
◦  Fixed the Near Velocity field output. 
◦  Increasing the limit of number of parts for the model. 
◦  Temperature added as a surface variable in output. 
◦  Fixed non-linear conjugate heat solver. 
•  Implicit 
◦  Fixed  Implicit  for  the  case  of  Multi-step  Linear  (*CONTROL_IMPLICIT_
GENERAL  with  NSOLVR = 1)  with  Intermittent  Eigenvalue  Computation 
(*CONTROL_IMPLICIT_EIGENVALUE with NEIG < 0). 
◦  Recent  fix  for  resultant  forces  for  Multi-step  Linear  cause  segmentation 
fault when Intermittent Eigenvalue Computation was also active. 
◦  Fix  possible  issue  related  to  constrained  contacts  in  MPP  implicit  not  ini-
tializing properly. 
◦  Fixed label at beginning of implicit step to be correct for the case of control-
load  curve  (*CONTROL_IMPLICIT_
implicit  dynamics  via  a 
ling 
DYNAMICS). 
◦  Corrected  the  computation  of  modal  stresses  with  local  coordinate  terms 
and  forsome  shell  elements  . 
◦  Corrected  *CONTROL_IMPLICIT_INERTIA_RELIEF  logic  in  MPP.    In 
some cases the rigid body modes were lost. 
◦  Enhanced  implicit's  treatment  of  failing  spotwelds  (*CONSTRAINED_
SPOTWELD).
INTRODUCTION 
◦  Added additional error checking of input data for *CONTROL_IMPLICIT_
MODAL_DYNAMICS_DAMPING. 
◦  Per  user  request  we  added  the  coupling  of  prescribed  motion  constraints 
for  Modal  Dynamics  by  using  constraint  modes.    See  *CONTROL_
IMPLICIT_MODAL_DYNAMIC. 
◦  Added  reuse  of  the  matrix  reordering  for  MPP  implicit  execution.    This 
will  reduce  the  symbolic  processing  time  which  is  noticable  when  using 
large numbers of MPP processes.  Also added prediction of non tied con-
tact  connections  for  standard  contact  and  mortar  contact.    This  allows  re-
use of the ordering when contact interfaces are changing very slightly but 
can  increase  the  cost  of  the  numerical  factorization.    Useful  only  for  MPP 
using large numbers of processes for large finite element models.  This re-
use checking happens automatically for MPP and is not required for SMP. 
◦  Apply  improvements  to  Metis  memory  requirements  used  in  Implicit 
MPP. 
◦  Enhanced  Metis  ordering  software 
(ORDER = 2, 
the  default,  on 
*CONTROL_IMPLICIT_SOLVER). 
◦  Added  new  keyword  *CONTROL_IMPLICIT_ORDERING  to  control  of 
features of the ordering methods for the linear algebra solver in MPP Im-
plicit.  Only should be used by expert users. 
◦  The  following  4  enhancements  are  applicable  when  IMFLAG > 1  on 
*CONTROL_IMPLICIT_GENERAL. 
  Implicit  was  modified  to  reset  the  time  step  used  in  contact  when 
switching from implicit to explicit. 
  Adjusted implicit mechanical time step for the case of switching from 
explicit to implicit so as not to go past the end time. 
  Explicit  with  intermittent  eigenvalue  analysis  was  getting  incorrect 
results  after  the  eigenvalue  analysis  because  an  incorrect  time  step 
was  used  for  the  implicit  computations.  For  this  scenario  implicit 
now uses the explicit time step. 
  The  implicit  time  step  is  now  reset  for  the  dump  file  in  addition  to 
explicit's time. 
◦  Implicit's treatment of prescribed motion constraints defined by a box had 
to be enhanced to properly handle potential switching to explicit. 
◦  The  following  6  enhancements  are  for  matrix  dumping  (MTXDMP > 0  on 
response 
frequency 
for 
*CONTROL_IMPLICIT_SOLVER) 
(*FREQUENCY_DOMAIN) computations. 
or 
◦  Corrected  the  collection  of  *DAMPING_PART_STIFFNESS  terms  for  ele-
ments like triangles and 5, 6, and 7 node solid elements. 
◦  Corrected  Implicit's  access  of  *DAMPING_PART_STIFFNES  parameter 
when triangle and tet sorting is activated. 
◦  Fixed Implicit's collecting of damping terms for beams that have reference 
nodes.
INTRODUCTION 
◦  There  is  an  internal  switch  that  turns  off  damping  for  beams  if  the  run  is 
implicit static.  This switch needed to be turned off for explicit with inter-
mittent eigenvalue analysis. 
◦  Fixed  collecting  of  stiffness  damping  terms  for  implicit.    Corrected  the 
loading  of  mass  damping  terms  when  collecting  damping  terms  for  post 
processing. 
◦  Extend  matrix  dumping  to  include  dumping  the  solution  vector  in  addi-
tion to the matrix and right-hand-side. 
◦  Adjusted Implicit's handling of sw1.  and sw3.  sense switches to properly 
handle dumping.  If sw1.  sense switch is issued when not at equilibrium, 
then reset time and geometry to that at the end of last implicit time step.  If 
sw3.  sense switch is issued, then wait until equilibrium is reached before 
dumping and continuing. 
◦  Enable  the  use  of  intermittent  eigenvalue  computation  for  models  using 
inertia  relief  and/or  rotational  dynamics.    See  NEIG < 0  on  *CONTROL_
IMPLICIT_EIGENVALUE 
and 
*CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS.    Due  to  round-off, 
an implicit intermittent eigenvalue computation was occasionally skipped.  
A  fudge  factor  of  1/1000  of  the  implicit  time  step  was  added  to  compen-
sate  for  round-off  error  in  the  summation  of  the  implicit  time.    See 
NEIG < 0 on *CONTROL_IMPLICIT_EIGENVALUE. 
*CONTROL_INERTIA_RELIEF 
and 
◦  Added  support  for  *CONSTRAINED_LINEAR  for  2D  implicit  problems.  
It was already supported for standard 3D problems. 
◦  Added  warning  for  implicit  when  the  product  of  ILIMIT  and  MAXREF 
(two parameters on *CONTROL_IMPLICIT_SOLUTION) is too small.  For 
the special case when the user changes the default of ILIMIT to 1 to choose 
Full Newton and does not change MAXREF then MAXREF is reset to 165 
and a warning is generated.  Reinstate the option of MAXREF < 0. 
◦  Fixed  the  display  of  superelements  in  LS-PrePost.    Enhanced  reading  of 
Nastran dmig files to allow for LS-DYNA-like  comment lines starting with 
'$'.  Fixed a problem with implicit initialization in MPP with 2 or more su-
perelements.  See *ELEMENT_DIRECT_MATRIX_INPUT. 
◦  Turned  off  annoying  warning  messages  associated  with  zero  contact  ele-
mental stiffness matrices coming from mortar contact.  See *CONTACT_..._
MORTAR 
◦  Fixed construction of d3mode file in MPP.  Involves proper computation of 
the reduced stiffness matrix.  See *CONTROL_IMPLICIT_MODES 
◦  Fixed up *PART_MODES to correctly handle constraint modes. 
  removed rigid body modes 
  correct construction of reduced stiffness matrix 
◦  Enhanced the error handling for input for *PART_MODES. 
◦  Modified open statements for binary files used by implicit to allow for use 
of *CASE.
INTRODUCTION 
◦  Removed  internal  use  files  such  as  spooles.res  when  not  required  for  de-
bugging. 
◦  Fixed  implicit  static  condensation  and  implicit  mode  computation  to 
properly  deal  with  the  *CASE  environment.   See  *CONTROL_IMPLICIT_
STATIC_CONDENSATION  and  *CONTROL_IMPLICIT_MODES.    Sort 
node/dof  sets  for  implicit_mode  to  get  correct  results.    Properly  handle 
cases with only solid elements. 
◦  Add implicit implementation of the new "last location" feature for MPP er-
ror tracking. 
◦  Fixed problem with implicit processing of rigid body data with deformable 
to rigid switching (*DEFORMABLE_TO_RIGID). 
◦  Extended  Implicit  model  debugging  for  LPRINT = 3  (*CONTROL_
IMPLICIT_SOLVER) to isogeometric and other large elemental stiff matri-
ces. 
◦  Added beam rotary mass scaling to the modal effective mass computation.  
Enhanced  implicit  computation  of  modal  effective  mass  that  is  output  to 
file  eigout  with  *CONTROL_IMPLICIT_EIGENVALUE.    We  had  to  ac-
count for boundary SPC constraints as well as beam reference nodes to get 
the accumulated percentage to add up to 100%. 
◦  Fixed a problem reporting redundant constraints for MPP Implicit. 
◦  Enhanced *CONTACT_AUTO_MOVE for implicit. 
◦  Fixed Implicit handling of *CONSTRAINED_TIE-BREAK in MPP. 
◦  Added support for implicit dynamics to *MAT_157 and *MAT_120. 
◦  Skip frequency damping during implicit static dynamic relaxation. 
◦  Added feature to simulate brake squeal.  Transient and mode analysis can 
be combined to do the brake squeal study by intermittent eigenvalue anal-
ysis. 
*CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS, 
*CONTROL_IMPLICIT_SOLVER should also be used, setting LCPACK = 3 
to enable unsymmetric stiffness matrix.  In the non-symmetric stiffness ma-
trix analysis such as brake squeal analysis, the damping ratio, defined as -
2.0*RE(eigenvalue)/ABS(IMG(eigenvalue)), can be output to the eigout file 
and plotted in LS-PrePost.  A negative damping ratio indicates an unstable 
mode. 
  Besides 
◦  Add a warning message if the defined rotational speed is not the same as 
NOMEG in *CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS. 
◦  *CONTROL_IMPLICIT:  Fixed  a  bug  to  initialize  velocity  correctly  when 
using a displacement file in dynamic relaxation for implicit MPP. 
◦  Nonlinear implicit solver 12 is made default implicit solver, which is aimed 
for enhanced robustness in particular relation to BFGS and line search. 
◦  Parameter  IACC  available  on  *CONTROL_ACCURACY  to  invoke  en-
hanced accuracy in selected elements, materials and tied contacts.  Includ-
ed is strong objectivity in the most common elements, strong objecitity and 
physical respons in most commont tied contacts and full iteration plasticity 
in *MATs 24 and 123.  For more detailed information refer to the manual.
INTRODUCTION 
◦  Bathe composite time integration scheme implemented for increased stabil-
ity  and  conservation  of  energy/momentum,  see  *CONTROL_IMPLICIT_
DYNAMICS. 
  Time  integration  parameter  ALPHA  on  CONTROL_
IMPLICIT_DYNAMICS is used for activation. 
◦  For  NLNORM.LT.0  all  scalar  products  in  implicit  are  with  respect  to  all 
degrees  of  freedom,  sum  of  translational  and  rotational  (similar  to 
NLNORM.EQ.4), 
the  rotational  dofs  are  scaled  using 
ABS(NLNORM)  as  a  characteristic  length  to  appropriately  deal  with  con-
sistency of units. 
that 
just 
◦  The message 'convergence prevented due to unfulfilled bc...' has annoyed 
users.  Here this is loosened up a little and also accompanied with a check 
that the bc that prevents convergence is actually nonzero.  Earlier this pre-
vention  has  activated  even  for  SPCs  modelled  as  prescribed  zero  motion, 
which does not make sense. 
◦  Implicit now writes out the last converged state to the d3plot database on 
error termination if not already written. 
◦  Fixed  bug  for  *CONTROL_IMPLICIT_MODAL_DYNAMIC  if  jobid  is 
used. 
•  *INITIAL 
◦  Fix incorrect NPLANE and NTHICK for *INITIAL_STRESS_SHELL when 
output to dynain file for shell type 9. 
◦  Fix *INITIAL_STRAIN_SHELL output to dynain for shell types 12 to 15 in 
2D analysis. 
◦  Write  out  strain  at  only  1  intg  point  if  INTSTRN = 0  in  *INTERFACE_
SPRINGBACK_LSDYNA and all strains at all 4 intg points if INTSTRN = 1 
and nip = 4 in *SECTION_SHELL. 
◦  *INITIAL_EOS_ALE:  Allow  initialization  of  internal  energy  density,  rela-
tive volume, or pressure in ALE elements by part, part set, or element set. 
◦  *INITIAL_VOLUME_FRACTION_GEOMETRY: Add option (FAMMG < 0) 
to  form  pairs  of  groups  in  *SET_MULTI-MATERIAL_GROUP_LIST  to  re-
place the first group of the pair by the second one. 
◦  *INITIAL_STRESS_DEPTH  can  now  work  with  parts  that  have  an  Equa-
tion  of  State  (EOS  types  1,  4,  6  only).    Note  however  that  *INITIAL_
STRESS_DEPTH does not work with ALE. 
◦  Fix  several  instances  of  overwriting  the  initial  velocities  of  any  interface 
nodes read in from a linking file (SMP only). 
◦  *INITIAL_VOLUME_FRACTION_GEOMETRY:  Add  local  coordinate  sys-
tem option for box. 
◦  The 
initial  strain  and  energy 
is  calculated  for  *INITIAL_FOAM_
REFERENCE_GEOMETRY. 
◦  Add  the  option  of  defining  the  direction  cosine  using  two  nodes  for 
*INITIAL_VELOCITY_GENERATION.
INTRODUCTION 
◦  Fix  incorrect  transformation  of  *DEFINE_BOX  which  results  in  incorrect 
initial velocities if the box is used in *INITIAL_VELOCITY. 
◦  Fix incorrect initial velocity when using *INITIAL_VELOCITY with NX = -
999. 
◦  Fix  seg  fault  when  using  *INITIAL_INTERNAL_DOF_SOLID_TYPE4  in 
dynain file. 
◦  Do  not  transform  the  translational  velocities  in  *INITIAL_VELOCITY  or 
*INITIAL_VELOCITY_GENERATION  if  the  local  coordinate  system  ICID 
is defined. 
◦  Fix  uninitialized 
*INITIAL_VELOCITY_
GENERATION  with  STYP = 2,  i.e.    part  id,  for  *ELEMENT_SHELL_
COMPOSITE/*ELEMENT_TSHELL_COMPOSITE. 
velocities  when  using 
◦  Fix  incorrect  initialization  of  velocities  if  using  *INITIAL_VELOCITY_
GENERATION with STYP = 1, i.e.  part set for shells with formulation 23 
& 24. 
◦  Fix incorrect initial velocity and also mass output to d3hsp for shell types 
23 & 24. 
◦  Fix 
incorrect 
initial  velocities  when  using  *INITIAL_VELOCITY_
GENERATION  with  irigid = 1  and  *PART_INERTIA  with  xc = yc = zc = 0 
and nodeid > 0 with *DEFINE_TRANSFORMATION. 
◦  Fix  incorrect  stress  initialization  of  *MAT_057/MAT_LOW_DENSITY_
FOAM  using  dynain  file  with  *INITIAL_STRESS_SOLID  when  NHISV  is 
equal to the number of history variables for this mat 57. 
◦  Fix seg fault when reading dynain.bin 
◦  Fixed stress initialization (*INITIAL_STRESS_SECTION) for type 13 tetra-
hedral  elements.    The  pressure  smoothing  was  causing  incorrect  pressure 
values in the elements adjacent to the prescribed elements. 
◦  Assign  initial  velocities  (*INITIAL_VELOCITY)  to  beam  nodes  that  are 
generated  when  release  conditions  are  defined  (RT1,  RT2,  RR1,  RR2  on 
*ELEMENT_BEAM.) 
◦  Added an option to retain bending stiffness in spot weld beams that have 
prescribed  axial  force.    To  use  is,  set  KBEND = 1  on  *INITIAL_AXIAL_
FORCE_BEAM. 
◦  Fix  for  *INITIAL_STRESS_BEAM  when  used  with  spotweld  beam  type  9.  
It  was  possible  that  error/warning  message  INI+140  popped  up  even  if 
number of integration points matched exactly. 
◦  Fix  for  the  combination  of  type  13  tet  elements  and  *INITIAL_STRESS_
SOLID.  The necessary nodal values for averaging (element volume, Jaco-
bian)  were  not  correctly  initialized.    Now  the  initial  volume  (IVEFLG)  is 
used to compute the correct initial nodal volume. 
•  Isogeometric Elements 
◦  Enable spc boundary condition to be applied to extra nodes of nurbs shell, 
see *CONSTRAINED_NODES_TO_NURBS_SHELL
INTRODUCTION 
◦  Fix  a  bug  for  isogeometric  element  contact,  IGACTC = 1,  that  happens 
when more than one NURBS patches are used to model a part so that a in-
terpolated elements have nodes belonging to different NURB patches. 
◦  *ELEMENT_SOLID_NURBS_PATCH: 
  Enable  isogeometric  analysis  for  solid  elements,  it  is  now  able  to  do 
explicit and implicit analysis, such as contact and eigenvalue analysis, 
etc. 
  Add mode stress analysis for isogeometric solid and shell elements so 
that  the  isogeometric  element  is  also  able  to  do  frequency  domain 
analysis. 
◦  Add  reduced,  patch-wise  integration  rule  for  C1-continuous  quadratic 
NURBS.    This  can  be  used  by  setting  INT = 2  in  *ELEMENT_SHELL_
NURBS_PATCH. 
◦  Add  trimmed  NURBS  capability.    Define  NL  trimming  loops  to  specify  a 
trimmed  NURBS  patch.    Use  *DEFINE_CURVE  (DATTYP = 6)  to  specify 
define trimming edges in the parametric space. 
◦  Fix bug in added mass report for *ELEMENT_SHELL_NURBS_PATCH in 
MPP. 
•  *LOAD 
◦  *LOAD_GRAVITY_PART  and  staged  construction  (*DEFINE_STAGED_
CONSTRUCTION_PART)  were  ignoring  non-structural  mass  MAREA 
(shells) and NSM (beams).  Now fixed. 
◦  Fix for *INTERFACE_LINKING in MPP  when used with adaptivity. 
◦  Updates  for  *INTERFACE_LINKING  so  that  it  can  be  used  with  adaptiv-
ity, provided the linked parts are adapting. 
◦  Fix for *INTERFACE_LINKING when  used  with LSDA based  files gener-
ated by older versions of the code. 
◦  *DEFINE_CURVE_FUNCTION: 
  Functions "DELAY", PIDCTL" and "IF" of are revised. 
  Add  sampling  rate  and  saturation  limit  to  PIDCTL  of  *DEFINE_
CURVE_FUNCTION. 
  "DELAY" of *DEFINE_CURVE_FUNCTION can delay the value of a 
time-dependent curve by "-TDLY" time steps when TDLY < 0. 
◦  Add edge loading option to *LOAD_SEGMENT_SET_NONUNIFORM. 
◦  Fix  insufficient  memory  error,SOL+659,  when  using  *LOAD_ERODING_
PART_SET with mpp. 
◦  Fix  incorrect  loading  when  using  *LOAD_ERODING_PART_SET  with 
BOXID defined.
INTRODUCTION 
◦  Fix  incorrect  pressure  applied  if  the  directional  cosines,  V1/V2/V3,  for 
*LOAD_SEGMENT_SET_NONUNIFORM do not correspond to a unit vec-
tor. 
◦  Add  *DEFINE_FUNCTION  capability  to  *LOAD_SEGMENT_SET  for  2D 
analysis. 
◦  Fix  incorrect  behavior  when  using  arrival  time,  AT,  or  box,  BOXID,  in 
*LOAD_ERODING_PART_SET. 
◦  Fix  error  when  runing  analysis  with    *LOAD_THERMAL_CONSTANT_
ELEMENT_(OPTION) in MPP with ncpu > 1. 
◦  Fixed  *LOAD_STEADY_STATE_ROLLING  when  used  with  shell  form  2 
when  used  with  Belytschko-Wong-Chang  warping  stiffness  (BWC = 1 
*CONTROL_SHELL). 
◦  Add  "TIMESTEP"  as  a  code  defined  value  available  for  *DEFINE_
FUNCTION  and  *DEFINE_CURVE_FUNCTION.    It  holds  the  current 
simulation timestep. 
◦  Fixed issues involving *LOAD_THERMAL_D3PLOT. 
◦  Allow extraction of node numbers in loadsetud for all values of LTYPE in 
*USER_LOADING_SET.    Comments  included  appropriately  in  the  code.  
Argument list of loadsetud is changed accordingly. 
◦  Implemented SPF simulation (*LOAD_SUPERPLASTIC_FORMING) for 2d 
problems. 
◦  Added effective stress as target variable for SPF simulation. 
◦  Added box option for SPF simulation to limit target search regions. 
•  *MAT 
◦  Fix  output  to  d3hsp  for  *MAT_HYPERELASTIC_RUBBER.    Broken  in 
r93028. 
◦  Error  terminate  with  message,  KEY+1115,  if_STOCHASTIC  option  is  in-
voked  for  *MATs  10,15,24,81,98,  123  but  no  *DEFINE_STOCHASTIC_
VARIATION  or  *DEFINE_HAZ_PROPERTIES  keyword  is  present  in  the 
input file. 
◦  Fix  spurious  error  termination  when  using  *DEFINE_HAZ_PROPERTIES 
with adaptivity. 
◦  Fixed *MATs 161 and 162 when run with MPP.  The array that is used to 
share delamination data across processors had errors. 
◦  *MAT_261/*MAT_262:  Fixed  problem  using 
*DAMPING_PART_
STIFFNESS together with RYLEN = 2 in *CONTROL_ENERGY. 
◦  Added safety check for martensite phase kinetics in *MAT_244. 
◦  Fix  for  combination  of  *MAT_024_STOCHASTIC  and  shell  elementstype 
13, 14, and 15 (with 3d stress state). 
◦  Fix  bug  in  *MATs  21  and  23  when  used  with  *MAT_ADD_THERMAL_
EXPANSION. 
◦  *MAT_ALE_VISCOUS:  Implement  a  user  defined  routine  in  dyn21.F  to 
compute the dynamic viscosity.
INTRODUCTION 
◦  Add histlist.txt to usermat package.  This file lists the history variables by 
material. 
◦  Bug in *MAT_089 fixed: The load curve LCSS specifies the relationship be-
tween "maximum equivalent strain" and the von Mises stress.  The "maxi-
mum equivalent strain" includes both elastic and plastic components.  The 
material  model  was  not  calculating  this  variable  as  intended,  so  was  not 
following  LCSS  accurately.    The  error  was  likely  to  be  more  noticeable 
when elastic strains are a significant proportion of the total strain e.g.  for 
small strains or low initial Youngs modulus. 
◦  Fixed bug affecting *MAT_119: unpredictable unloading behaviour in local 
T-direction  if  there  are  curves  only  for  the  T-direction  and  not  for  the  S-
direction. 
◦  Fixed  bug  in  *MAT_172:  Occured  when  ELFORM = 1  (Hughes-Liu  shell 
formulation)  was  combined  with  Invariant  Numbering  (INN > 0  on 
*CONTROL_ACCURACY).  In this case, the strain-softening in tension did 
not work: after cracking, the tensile strength remained constant. 
◦  New option for *MAT_079: Load curve LCD defining hysteresis damping 
versus maximum strain to date.  This overrides the default Masing behav-
iour. 
◦  *MAT_172: 
  Added  error  termination  if  user  inputs  an  illegal  value  for  TYPEC.  
Previously,  this  condition  could  lead  to  abnormal  terminations  that 
were difficult to diagnose. 
  Fixed bug affecting ELFORM = 16 shells made of *MAT_172 – spuri-
ous strains could develop transverse to the crack opening direction. 
◦  Fixed bug in *MAT_ARUP_ADHESIVE (*MAT_169).  The displacement to 
failure in tension was not as implied by the inputs TENMAX and GCTEN.  
For  typical  structural adhesives  with  elastic  stiffness  of  the  order of  1000-
10000  MPa,  the  error  was  very  small.    The  error  became  large  for  lower 
stiffness materials. 
◦  *MAT_SPR_JLR: 
  Modify output variables from *MAT_SPR_JLR . 
  Fix bug that caused spurious results or unexpected element deletion 
if TELAS = 1. 
◦  Fixed  bug  in  *MAT_174  -  the  code  could  crash  when  input  parameters 
EUR = 0 and FRACR = 0.. 
◦  Fix MPP problem when writing out aea_crack file for *MAT_WINFRITH. 
◦  Include *MAT_196 as one that triggers spot weld thinning. 
◦  *MAT_ADD_FATIGUE: Implemented multi slope SN curves to be used in 
(*FREQUENCY_DOMAIN_RANDOM_
vibration 
random 
fatigue
INTRODUCTION 
VIBRATION_FATIGUE)  and  SSD  fatigue  (FREQUENCY_DOMAIN_SSD_
FATIGUE). 
◦  Guard against possible numerical round off that in some cases might result 
in unexpected airflow in *MAT_ADD_PORE_AIR. 
◦  Added new material *MAT_115_O/*MAT_UNIFIED_CREEP_ORTHO. 
◦  *MAT_274: Added support for 2D-solids.  New flag (parameter 8 on card 
2) is used to switch normal with in-plane axis. 
◦  *MAT_255: Fixed bug in plasticity algorithm and changed from total strain 
rate  to  plastic  strain  rate  for  stability.    Added  VP  option  (parameter  5  on 
card  2)  for  backwards  compatibility:  VP = 0  invokes  total  strain  rate  used 
as before. 
◦  Added  new  cohesive  material  *MAT_279/*MAT_COHESIVE_PAPER  to 
be used in conjunction with *MAT_274/*MAT_PAPER. 
◦  User  materials:  Added  support  for  EOS  with  user  materials  for tshell  for-
mulations 3 and 5. 
◦  Fixed bug in dyna.str when using EOS together with shells and orthotropic 
materials. 
◦  *MAT_122: A new version of *MAT_HILL_3R_3D is available.  It supports 
temperature  dependent  curves  for  the  Young's/shear  moduli,  Possion  ra-
tios,  and  Hill's  anisotropy  parameters.   It  also  supports  2D-tables  of  yield 
curves  for  different  temperatures.    Implicit  dynamics  is  supported.    The 
old version is run if parameter 5 on card 3 is set to 1.0. 
◦  Added  the  phase  change  option  to  *MAT_216,  *MAT_217,  *MAT_218  to 
allow material properties to change as a function of location.  This capabil-
ity is designed to model materials that change their properties due to ma-
terial  processing  that  is  otherwise  not  modeled.    For  example,  increasing 
the mass and thickness due to the deposition of material by spraying.  It is 
not used for modeling phase changes caused by pressure, thermal loading, 
or other mechanical processes modeled within LS-DYNA. 
◦  Fix  internal  energy  computation  of  *MAT_ELASTIC_VISCOPLASTIC_
THERMAL/MAT_106. 
◦  Fix incorrect results or seg fault for *MAT_FU_CHANG_FOAM/MAT_083 
if KCON > 0.0 and TBID.ne.0. 
◦  If  SIGY = 0  and  S = 0  in  *MAT_DAMAGE_2/MAT_105,  set  S = EPS1/200, 
where EPS1 is the first point of yield stress input or the first ordinate point 
of the LCSS curve. 
◦  Set  xt = 1.0E+16  as  default  if  user  inputs  0.0  for  *MAT_ENHANCED_
COMPOSITE_DAMAGE/MAT_054.    Otherwise,  random  failure  of  ele-
ments may occur.  Implemented for thick shells and solids. 
◦  Allow  *MAT_ENHANCED_COMPOSITE_DAMAGE/MAT_054 
failure 
mechanism to work together with *MAT_ADD_EROSION for shells. 
◦  Fix incorrect erosion behavior if *MAT_ADD_EROSION is used with fail-
*MAT_123/MAT_MODIFIED_PIECEWISE_
for 
ure  criteria  defined 
LINEAR_PLASTICITY.
INTRODUCTION 
◦  Fix non-failure of triangular elements type 4 using *MAT_ADD_EROSION 
with NUMFIP = -100. 
◦  Implement  scaling  of  failure  strain  for  *MAT_MODIFIED_PIECEWISE_
for 
LINEAR_PLASTICITY_STOCHASTIC/MAT_123_STOCHASTIC 
shells. 
◦  Fix 
incorrect  behavior 
*MAT_LINEAR_ELASTIC_DISCRETE_
BEAM/MAT_066  when  using  damping    with  implicit(statics)  to  explicit 
switching. 
for 
◦  Fix error due to convergence when using *MAT_CONCRETE_EC2/MAT_
172 in implicit and when FRACRX = 1.0 or FRACRY = 1.0 
◦  Fix  incorrect  fitting  results  for  *MAT_OGDEN_RUBBER/MAT_077_O  if 
the number of data points specifed in LCID is > 100. 
◦  Fix incorrect fitting results for *MAT_MOONEY-RIVLIN-RUBBER/MAT_
027 if the number of data points specifed in LCID is > 100. 
◦  Fix  incorrect  forces/moments  when  preloads  are  used  for  *MAT_
067/NONLINEAR_ELASTIC_DISCRETE_BEAM  and  the  strains  changes 
sign. 
◦  Implement 
*MAT_188/MAT_THERMO_ELASTO_VISCOPLASTIC_
CREEP for 2D implicit analysis. 
◦  Support  implicit  for  *MAT_121/MAT_GENERAL_NONLINEAR_1DOF_
DISCRETE_BEAM. 
◦  Fix  seg  fault  when  using  *DEFINE_HAZ_TAILOR_WELDED_BLANK 
with *DEFINE_HAZ_PROPERTIES. 
◦  Fix ineffective *MAT_ADD_EROSION if the MID is defined using a alpha-
numeric label. 
◦  Fix  seg 
fault  when  using 
THERMAL/MAT_255 for solids. 
*MAT_PIECEWISE_LINEAR_PLASTIC_
◦  Zero the pressure for *MAT_JOHNSON_HOLMQUIST_JH1/MAT_241 af-
ter it completely fractures, i.e.  D>=1.0, under tensile load. 
◦  Fix incorrect element failure when using EPSTHIN and VP = 0 for *MAT_
123/MODIFIED_PIECEWISE_LINEAR_PLASTICITY. 
◦  Fix error termination when using adaptive remeshing for 2D analysis with 
*MAT_015/JOHNSON_COOK  and  NIP = 4  in  *SECTION_SHELL  and 
ELFORM = 15. 
◦  Fix erosion due to damage, max shear & critical temperature in elastic state 
for *MAT_MODIFIED_JOHNSON_COOK/MAT_107 for solids. 
◦  Check 
diagonal 
elements 
{OPTION}TROPIC_ELASTIC  and 
STR+1306, if any of them are negative. 
of  C-matrix 
error 
*MAT_002/MAT_
terminate  with  message, 
of 
◦  Fix  plastic  strain  tensor  update  for  *MAT_082/*MAT_PLASTICITY_
WITH_DAMAGE. 
◦  Fix  error  when  using  *MAT_144/MAT_PITZER_CRUSHABLE_FOAM 
with solid tetahedron type 10. 
◦  Fix  out-of-range  forces  after  dynamic  relaxation  when  using  VP = 1  for 
*MAT_PIECEWISE_LINEAR_PLASTICITY  and  non-zero  strain  rate  pa-
INTRODUCTION 
rameters, C & P, and the part goes into plastic deformation during dynam-
ic relaxation. 
◦  Fixed  unit  transformation  for  GAMAB1  and  GAMAB2  on  *MAT_DRY_
FABRIC.  We were incorrectly transforming them as stress. 
◦  Fixed implicit solutions with shell elements that use *MAT_040 and lami-
nated shell theory. 
◦  Fixed the stress calculation in the thermal version of *MAT_077. 
◦  Corrected  the  AOPT = 0  option  of  ortho/anisotropic  materials  when  use 
with skewed solid elements.  Previously, the material direction was initial-
ized to be equivalent to the local coordinate system direction.  This is not 
consistent with the manual for skewed elements which states that the ma-
terial a-axis is in the 1-2 directions for AOPT = 0.  This is now fixed and the 
manual is correct. 
◦  Fixed  the  AOPT = 0  option  of  ortho/anisotropic  materials  for  tetrahedral 
element forms 10, 13, and 44. 
◦  Fixed *MAT_082 for solid elements.  An error in the history data was caus-
ing possible energy growth or loss of partially damaged elements. 
◦  Modified  *MAT_FABRIC/*MAT_034  FORM = 24  so  that  Poisson's  effects 
occur in tension only. 
◦  Modified  *MAT_221/*MAT_ORTHOTROPIC_SIMPLIFIED_DAMAGE  to 
correct the damage behavior.  Prior to this fix, damage was applied to new 
increments  of  stress,  but  not  the  stress  history,  so  material  softening  was 
not possible. 
◦  Fixed  *MAT_106  when  used  with  curves  to  define  the  Young's  modulus 
and  Poisson's  ratio  and  when  used  with  thick  shell  form  5  or  6.    The  as-
sumed strain field was unreasonable which caused implicit convergence to 
fail. 
◦  Added  2  new  erosion  criteria  for  *MAT_221/*MAT_ORTHOTROPC_
SIMPLIFIED_DAMAGE.  The new options are    NERODE = 10:  a or b di-
rections  failure  (tensile  or  compressive)  plus  out  of  plane  failure bc  or  ca.  
NERODE = 11:    a  or  b  directions  failure  (tensile  only)  plus  out  of  plane 
failure bc or ca. 
◦  Added a new option for shell *MAT_022/*MAT_COMPOSITE_DAMAGE.  
When  ATRACK = 1,  the  material  directions  will  follow  not  only  element 
rotation, but also deformation.  This option is useful for modeling layered 
composites, that have material a-directions that vary by layer, by allowing 
each layer to rotate independently of the others.  Within each layer, the b-
direction is always orthogonal to the a-direction. 
◦  Fixed  the  TRUE_T  option  on  *MAT_100  and  *MAT_100_DA.    If  the  weld 
connects  shells  with  different  thickness  and  therefore  different  bending 
stiffness,  the  scheme  used  by  TRUE_T  to  reduce  the  calculated  moment 
could  behave  somewhat  unpredictably.    With  the  fix,  TRUE_T  behaves 
much better, both for single brick welds and brick assemblies.
INTRODUCTION 
◦  Added  a  warning  message  and  automatically  switch  DMGOPT > 0  to 
DMGOPT = 0  on  *MAT_FABRIC  when  RS < EFAIL  or  RS = EFAIL.    This 
prevents a problem where weld assemblies did not fail at all when RS = 0. 
◦  *MATs 9, 10, 11, 15, 88, and 224 are now available for thick shells, however 
only *MATs 15, 88, and 224 are available for the 2D tshell forms 1,2, and 6. 
◦  Added  thick  shell  support  for  the  STOCHASTIC  option  of  *MATs  10,  15, 
24, 81, and 98. 
◦  Added  support  for  *MAT_096  for  several  solid  element  types  including 
ELFORMs 3, 4, 15, 18, and 23. 
◦  Added  a  MIDFAIL  keyword  option  for  *MAT_024,  (MAT_PIECEWISE_
LINEAR_PLASTICITY).    With  this  option,  element  failure  does  not  occur 
until the failure strain is reached in the mid plane layer.  If an even number 
of layers is used, then the failure occurs when the 2 closest points reach the 
failure strain. 
◦  Enabled  *MATs  26  and  126  (HONEYCOMB)  to  be  used  with  thick  shell 
forms 3, 5, and 7.  These was initialized incorrectly causing a zero stress. 
◦  Enabled *MAD_ADD_EROSION to be used with beams that have user de-
fined integration. Memory allocation was fixed to prevent memory errors. 
◦  Enabled OPT = -1 on *MAT_SPOTWELD for solid elements. 
◦  Enabled  thick  shells  to  use  *MATs  103  and  104  in  an  implicit  solution. 
These  materials  were  lacking  some  data  initialization  so  they  would  not 
converge. 
◦  Enabled  solid  elements  with  user-defined  orthotropic  materials  to  work 
with  the  INTOUT  and  NODOUT  options  on  *DATABASE_EXTENT_
BINARY.  The transformation matrix was stored in the wrong place caus-
ing strain and stress transformations to fail. 
◦  Enabled *MAT_017 to run with thick shell forms 3 and 5.  Neither element 
was initialized correctly to run materials with equations of state. 
◦  Add degradation factors and strain rate dependent strength possibility for 
*MAT_054/*MAT_ENHANCED_COMPOSITE_DAMAGE solids. 
◦  Fixed  bug 
in  *MAT_058/*MAT_LAMINATED_COMPOSITE_FABRIC 
when  used  with  strain-rate  dependent  tables  for  stiffnesses  EA,  EB  and 
GAB and LAMSHT = 3. 
◦  Add strain rate dependency of ERODS in *MAT_058. 
◦  Add  possibility  to  use  *DEFINE_FUNCTION  for  *MAT_SPOTWELD_
DAMAGE_FAILURE  (*MAT_100),  OPT = -1/0.    If  FVAL = FunctionID, 
then  a  *DEFINE_FUNCTION  expression  is  used  to  determine  the  weld 
failure criterion using the following arguments: func (N_rr, N_rs, N_rt, M_
rr, M_ss, M_tt). 
◦  Store tangential and normal separation (delta_II & delta_I) as history vari-
ables 1&2 of *MAT_138/*MAT_COHESIVE_MIXED_MODE. 
◦  Add  second  normalized  traction-separation  load  curve  (TSLC2)  for  Mode 
II in *MAT_186/*MAT_COHESIVE_GENERAL.
INTRODUCTION 
◦  Fixed  bug 
in  using 
*MAT_157/*MAT_ANISOTROPIC_ELASTIC_
PLASTIC with IHIS.gt.0 for shells.  Thickness strain update d3 was not cor-
rect and plasticity algorithm failed due to typo. 
◦  Fixed  bug  in  *MAT_157  for  solids:  This  affected  the  correct  stress  trans-
in  *DATABASE_
formation  for  post-processing  using  CMPFLG = 1 
EXTENT_BINARY. 
◦  Fixed  bug  in  *MAT_225  (*MAT_VISCOPLASTIC_MIXED_HARDENING) 
when using Table-Definition together with kinematic hardening. 
◦  Add  load  curves  for  rate  dependent  strengths  (XC,  XT,  YC,  YT,  SC)  in 
*MAT_261/*MAT_LAMINATED_FRACTURE_DAIMLER_PINHO  (shells 
only). 
◦  Add table definition for LCSS for rate dependency in *MAT_261 (shells on-
ly). 
◦  Add load curves for rate dependent strengths (XC, XCO, XT, XTO, YC, YT, 
*MAT_262/*MAT_LAMINATED_FRACTURE_DAIMLER_
SC) 
CAMANHO (shells only). 
in 
◦  Fixed bug when using *MAT_261 or *MAT_262 solids (ELFORM = 2). 
◦  Add  load  curves  for  SIGY  and  ETAN  for  rate  dependency  of  *MAT_262 
(shells only) 
◦  *MAT_021_OPTION 
  Fixed  a  bug  for  defining  different  orientation  angles  through  the 
thickness of TSHELL elements (formulations 2 and 3) 
  Added new option CURING: 
  Two additional cards are read to define parameters for curing kinet-
ics.  Formulation is based on Kamal's model and considers one ODE 
for the state of cure. 
  State of cure does not affect the mechanical parameters of the materi-
al. 
  CTE's  for  othotropic  thermal  expansione  can  be  defined  in  a  table 
with respect to state of cure and temperature. 
  An orthotropic chemical shrinkage is accounted for. 
◦  *MAT_REINFORCED_THERMOPLASTICS_OPTION 
(*MAT_249_
OPTION): 
  Fiber shear locking can be defined wrt to the fiber angle or shear an-
gle. 
  Output of fiber angle to history variables. 
  Simplified input: Instead of always reading 8 lines, now the user only 
has to specify data for NFIB fibers. 
  Added fiber elongation to history variables in *MAT_249 for pospro-
cessing. 
  New Option UDFIBER (based on a user defined material by BMW):
INTRODUCTION 
•  Transversely  isotropic  hyperelastic  formulation  for  each  fi-
ber family . 
•  Anisotropic bending behavior based on modified transverse 
shear stiffnesses. 
•  Best suited for dry NCF's. 
◦  *MAT_GENERALIZED_PHASE_CHANGE (*MAT_254): 
  New material that is a generalized version of *MAT_244 with appli-
cation to a wider range of metals. 
  Up to 24 different phases can be included. 
  Between each of the phases, the phase transformation can be defined 
based on a list of generic transformation laws.  For heating JMAK and 
Oddy  are  implemented.    For  cooling  Koistinen-Marburger,  JMAK 
and Kirkaldy can be chosen. 
  Constant  parameters  for  the  transformations  are  given  as  2d  tables, 
parameters  depending  on  temperature  (rate)  or  phase  concentration 
employ 3d tables. 
  Plasticity  model  (temperature  and  strain  rate  dependent)  similar  to 
MAT_244. 
  Transformation induced strains. 
  TRIP algorithm included. 
  Temperature dependent mixture rules. 
  Parameter 'dTmax' that defines the maximum temperature increment 
within  a  cycle.    If  the  temperature  difference  at  a  certain  integration 
point is too high, local subcycling is performed. 
  Implemented  for  explicit/implicit  analysis  and  for  2d/3d  solid  ele-
ments. 
◦  *MAT_ADHESIVE_CURING_VISCOELASTIC (*MAT_277): 
  New  material  implementation  including  a  temperature  dependent 
curing process of epoxy resin based on the Kamal-Sourour-model. 
  Material formulation is based on *MAT_GENERAL_VISCOELASTIC. 
  Viscoelastic  properties  defined  by  the  Prony  series,  coefficients  as 
functions of state of cure. 
  Chemical  and  thermal  shrinkage  considered  (differential  or  secant 
formulations). 
  Available for shell and solid elements. 
  Can be used in combination with *MAT_ADD_COHESIVE. 
  Implemented for explicit and implicit analysis. 
  An incremental and a total stress calculation procedure available. 
◦  Enable *MAT_ADD_EROSION to be safely used with material models that 
have more than 69 history variables, for now the new limit is 119.
INTRODUCTION 
◦  Use  correct  element  ID  for  output of  failed  solid  elements  when  GISSMO 
(*MAT_ADD_EROSION) is used with *CONTROL_DEBUG. 
◦  Improve  performance  of  GISSMO  (*MAT_ADD_EROSION  with  ID-
AM = 1),  especially  when  used  with  *MAT_024,  no  other  failure  criteria, 
shell  elements,  and  DMGEXP = 1  or  2.    Allows  speed-up  of  10  to  20  per-
cent. 
◦  Add  new  keyword  *MAT_ADD_GENERALIZED_DAMAGE.    It  provides 
a very flexible approach to add non-isotropic (tensorial) damage to stand-
ard materials in a modular fashion.  Solely works with shell elements at the 
moment. 
◦  Correct  the  computation  of  effective  strain  for  options  ERODS < 0  in 
*MAT_058  (*MAT_LAMINATED_COMPOSITE_FABRIC)  and  EFS < 0  in 
*MAT_261 
(*MAT_LAMINATED_FRACTURE_
DAIMLER_...).  The shear strain term was twice the size as it should have 
been. 
*MAT_262 
and 
◦  Adjust  stiffness  for  time  step  calculation  in  *MAT_076  and  subsequent 
models (*MAT_176, *MAT_276, ...) to prevent rarely observed instabilities. 
◦  Add  output  of  original  and  fitted  curves  to  messag  and  separate  file 
(curveplot_<MID>) for *MAT_103. 
◦  In  *MAT_104  (*MAT_DAMAGE_1),  stress-strain  curve  LCSS  can  now  be 
used directly with all FLAG options (-1,0,1,10,11), no fitting. 
◦  Correct  strain  calculation  for  anisotropic  damage  in  *MAT_104  (*MAT_
DAMAGE_1) with FLAG = -1. 
◦  Initialize  stress  triaxiality  of  *MAT_107  (*MAT_MODIFIED_JOHNSON_
COOK) to zero instead of 1/3. 
◦  Avoid  negative  damage  in  *MAT_107  (*MAT_MODIFIED_JOHNSON_
COOK) with FLAG2 = 0 for solid elements. 
◦  Rectify the characteristic element length in *MAT_138 (*MAT_COHESIVE_
MIXED_MODE) for solids type 21 and 22 (cohesive pentas) and shell type 
29 (cohesive shell) for "curve" options T < 0 and S < 0. 
◦  Correct/improve  material  tangent  for  *MAT_181  with  PR > 0  (foam  op-
tion). 
◦  Add  possibility  to  define  logarithmically  defined  strain  rate  table  LCID-T 
in material *MAT_187 (*MAT_SAMP-1). 
◦  Fix  missing  offset  when  using  *DEFINE_TRANSFORMATION  with  load 
curve LCID-P in *MAT_187 (*MAT_SAMP-1). 
◦  Add reasonable limit for biaxial strength in *MAT_187 with RBCFAC > 0.5 
to avoid concave yield surface. 
◦  Improve performance of *MAT_187 to reach speed-up of 10 to 40 percent, 
depending on which options are used. 
◦  Add new option for *MAT_224 (*MAT_TABULATED_JOHNSON_COOK).  
With BETA < 0 not only a load curve but now also a table can be referred 
to.    The  table  contains  strain  rate  dependent  curves,  each  for  a  different 
temperature.
INTRODUCTION 
◦  Fix  for  implicit  version  of  *MAT_224  (*MAT_TABULATED_JOHNSON_
COOK).  Computations with shell elements should converge faster now. 
◦  *MAT_224  (*MAT_TABULATED_JOHNSON_COOK)  can  now  be used  in 
implicit  even  with  temperature  dependent  Young's  modulus  (parameter 
E < 0). 
◦  Always  store  the  Lode  parameter  as  history  variable  #10  in  *MAT_224 
(*MAT_TABULATED_JOHNSON_COOK), not just for LCF being a table. 
◦  Variable LCI of *MAT_224 / *MAT_224_GYS can now refer to a *DEFINE_
TABLE_3D.  That means the plastic failure strain can now be a function of 
Lode  parameter  (TABLE_3D),  triaxiality  (TABLE),  and  element  size 
(CURVE). 
◦  For thick shells type 1 and 2, the element size in *MAT_224 is now correct. 
◦  Add  new  option  for  definition  of  parameters  FG1  and  FG2  in  *MAT_240 
(*MAT_COHESIVE_MIXED_MODE_ELASTOPLASTIC_RATE). 
◦  Add new option to *MAT_240: new load curves LCGIC and LCGIIC define 
fracture energies GIC and GIIC as functions of cohesive element thickness.  
GIC_0, GIC_INF, GIIC_0, and GIIC_INF are ignored in that case. 
◦  Add  new  feature  to  *MAT_248  (*MAT_PHS_BMW).    Estimated  Hocket-
Sherby  parameters  are  written  to  history  variables  based  on  input  func-
tions and phase fractions. 
◦  Add new option ISLC = 2 to *MAT_248 (*MAT_PHS_BMW) which allows 
to define load curves (cooling rate dependent values) for QR2, QR3, QR4, 
and all parameters on Cards 10 and 11. 
◦  Add  new  option  LCSS  to  *MAT_252  (*MAT_TOUGHENED_ADHESIVE_
POLYMER): A load curve, table or 3d table can now be used to define rate 
and temperature dependent stress-strain behavior (yield curve). 
◦  Fix  for  *MAT_255,  evaluation  of  2d  tables  LCIDC  and  LCDIT.    Negative 
temperatures were interpreted as logarithmic rates. 
◦  Add new material model *MAT_280 (*MAT_GLASS) for shell elements.  It 
is a  smeared fixed crack model with a selection of different brittle, stress-
state dependent failure criteria and crack closure effects. 
◦  *DEFINE_FABRIC_ASSEMBLIES:  Assemblies  of  *MAT_FABRIC  part  sets 
can be specified to properly treat bending of t-intersecting fabrics that are 
stitched  or  sewn  together.    See  ECOAT,  TCOAT  and  SCOAT  on  *MAT_
FABRIC_...  Bending can only occur within an assembly, aka a part set. 
◦  *MAT_USER_DEFINED_MATERIAL_MODELS:  In  user  defined  material 
models,  a  logical  parameter  'reject'  can  be  set  to  .true.    to  indicate  to  the 
implicit solver that equilibrium iterations should be aborted.  The criterion 
is  the  choise  of  the  implementor,  but  it  could  be  if  plastic  strain  increases 
by more than say 5% in one step or damage increases too much, whatever 
that might render an inaccurate prediction and bad results.  Setting this pa-
rameter for explicit won't do anything. 
◦  IHYPER = 3  for  user  shell  materials  now  supports  thickness  train  update, 
see *MAT_USER_DEFINED_MATERIAL_MODELS.
INTRODUCTION 
◦  *MAT_SIMPLIFIED_RUBBER/FOAM: AVGOPT < 0 is now supported for 
the  FOAM  option,  which  activates  a  time  averaged  strain  rate  scheme  to 
avoid noisy response. 
◦  MAT_181 is now supported for 2D implicit simulations. 
◦  *MAT_ADD_EROSION: 
  A  number  of  extensions  and  improvements  to  the  DIEM  damage 
model were made, IDAM < 0. 
  General efficiency, it was slow, now it's GOT to be faster. 
  NCS can be used as a plastic strain increment to only evaluate criteria 
in quantifications of plastic strain. 
  NUMFIP < 0  is  employing  the  GISSMO  approach,  number  of  layers 
for erosion. 
  A  new  ductile  damage  criterion  based  on  principal  stress  added 
(DMITYP = 4). 
  MSFLD and FLD can be evaluated in mid or outer layers to separate 
membrane and bending instability (P2). 
  MSFLD and FLD can use an incremental or direct update of instabil-
ity  parameter (P3). 
  Output of integration point failure information made optional (Q2). 
  Specifying DCTYP = -1 on the damage evolution card will not couple 
damage  to  stress  but  the  damage  variable  is  only  calculated  and 
stored. 
◦  *MAT_SMOOTH_VISCOELASTIC_VISCOPLASTIC,  *MAT_275:  An  elas-
tic-plastic model with  smooth transition between elastic and plastic mode 
is available.  It incorporates viscoelasticity and viscoplasticity and is based 
on  hyper-elastoplasticity  so  it  is  valid  for  arbitrarily  large  deformations 
and  rotations.   A  sophisticated  parameter  estimation  is  required  to match 
test data, it is available for implicit and explicit analyisis but perhaps most-
ly suited for implicit. 
◦  *MAT_FABRIC_MAP:  Stress  map  material  34  is  equipped  with  bending 
properties identical to that of the form 14 and form -14 version of the fab-
ric.    Coating  properties  are  set  in  terms  of  stiffness,  thickness  and  yield.  
The material is supported in implicit, including optional accounting for the 
nonsymmetric  tangent.    Should  be  used  with  bending  stiffness  on,  and 
convergence is improved dramatically if geometric stiffness is turned on. 
◦  *MAT_084 with predefined units (CONM < 0) is now transformed correct-
ly with INCLUDE_TRANSFORM. 
◦  If  LCIDTE = 0  in  *MAT_121,  then  LS-DYNA  was  crashing  on  some  plat-
forms, including Windows.  This is fixed. 
◦  Fix  initialization  issues  so  that  PML  models  can  be  run  with  *CASE  com-
mands. 
◦  *MAT_027 is revised to avoid accuracy issues for single precision executa-
bles.
INTRODUCTION 
◦  The nearly imcompressible condition is enhanced for *MAT_027 shell ele-
ments. 
◦  Add  a  new  material  model  as  a  option  for  *MAT_165.    *MAT_PLASTIC_
NONLINEAR_KINEMATIC_B  is  a  mixed  hardening  material  model,  and 
can be used for fatigue analysis. 
◦  Output  local  z-stress  in  *MAT_037,  when  *LOAD_STRESS_SURFACE  is 
used.  This was previously calculated and saved as another history varia-
ble. 
◦  Add a new material model *MAT_260 (2 forms). 
  Uses  non-associated  flow  rule  and  Hill's  yield  surface;  including 
strain rate effect and temperate effect.  MIT failure criteria is also im-
plemented. 
  Implemented for solids and shells. 
  Strain rate sensitivity for solids. 
  Option to directly input the Pij and Gij values. 
  Separate the material model *MAT_260 into *MAT_260A and *MAT_
260B: 
•  MAT260A=*MAT_STOUGHTON_NON_ASSOCIATED_
FLOW 
•  MAT260B=*MAT_MOHR_NON_ASSOCIATED_FLOW 
  Incorporates FLD into the fracture strain, so as to consider the mesh 
size effect. 
  Calculates the characteristic length of the element for *MAT_260B, so 
that an size-dependent failure criterial can be used. 
  When  failure  happens  for  half  of  the  integration  points  through  the 
thickness,  the element is deleted. 
◦  Add Formablitiy Index to *MAT_036, *MAT_037, *MAT_226. 
◦  Add  new  history  variables  for  Formability  Index,  affecting  *MAT_036, 
*MAT_037, *MAT_125, *MAT_226.  Those new history variables are FI, be-
ta, effective strain.  These comes after the 4 regular history variables. 
◦  *MAT_036, *MAT_125: New option_NLP is added to evaluate formability 
under non-linear strain paths.  User inputs a forming limit diagram (FLD), 
and  Formablitiy  Index  (F.I.)  will  be  automatically  converted  to  effective 
stain vs.  beta based space. 
•  MPP 
◦  Fix problem of MPP pre-decomposition that can occur if the local directory 
specified in the pfile has very different lengths in the initial run vs the ac-
tual run The difference resulted in a line count difference in the size of the 
structured  files  created,  throwing  off  the  reading  of  the  file  in  the  actual 
run. 
◦  Straighten out some silist/sidist issues in MPP decomp:
INTRODUCTION 
  silist  and  sidist  outside  of  a  "region"  in  the  pfile  are  no  longer  sup-
ported, and an error message is issued which suggests the use of "re-
gion { silist" instead. 
  They have been undocumented for several years (since "region" was 
introduced), and had other issues. 
◦  Fix 
the  keywords,  CONTROL_MPP_DECOMPOSITION_CONTACT_
and  CONTROL_MPP_DECOMPOSITION_CONTACT_
DISTRIBUTE 
ISOLATE,  which  were  not  treating  each  contact  interface  individually  (as 
the manual states), but collectively. 
◦  Fix for MPP decomp of part sets. 
◦  Fixed *CONTROL_MPP_PFILE (when used inside an include file) so that it 
honors ID offsets from *INCLUDE_TRANSFORM for parts, part sets, and 
contact ids referenced in "decomp { region {" specifications.  Furthermore, 
such  a  region  can  contain  a  "local"  designation,  in  which  case  the  decom-
position of that region will be done in the coordinate system local to the in-
clude file, not the global system.  For example: 
*CONTROL_MPP_PFILE 
decomp { region {partset 12 local c2r 30 0 -30 0 1 0 1 0 0}} 
would apply the c2r transformation in the coordinate system of the include 
file, which wasn't previously possible.  The local option can be useful even 
if there are no such transformations, as the "cubes" the decomposition uses 
will be oriented in the coordinate system of the include file, not the global 
system.  Furthermore, the following decomposition related keywords now 
have a_LOCAL option, which has the same effect: 
  *CONTROL_MPP_DECOMPOSITION_PARTS_DISTRIBUTE_
LOCAL 
  *CONTROL_MPP_DECOMPOSITION_PARTSET_DISTRIBUTE_
LOCAL 
  *CONTROL_MPP_DECOMPOSITION_ARRANGE_PARTS_LOCAL 
  *CONTROL_MPP_DECOMPOSITION_CONTACT_DISTRIBUTE_
LOCAL 
◦  Revert revision 86884, which was: 
  "MPP:  change  to  the  decomposition  behavior  of  *CONTROL_MPP_
DECOMPOSITION_PARTS_DISTRIBUTE 
*CONTROL_MPP_DECOMPOSITION_PARTSET_DISTRIBUTE 
*CONTROL_MPP_DECOMPOSITION_ARRANGE_PARTS 
in the case where a decomposition transformation is also used. Previ-
ously, any such regions were distributed without the transformation 
being applied.  This has been fixed so that any given transformation 
applies  to  these  regions  also.  So  now  the  transformations  will  NOT
INTRODUCTION 
apply to these keywords.  Really, the "region" syntax should be used 
together with *CONTROL_MPP_PFILE as it is more specific. 
◦  Modify behavior of DECOMPOSITION_AUTOMATIC so that if the initial 
velocity used is subject to *INCLUDE_TRANSFORM, the transformed ve-
locities are used. 
◦  Fix MPP decomposition issue with "decomp { automatic }" which was not 
honored when in the pfile. 
◦  Save hex weld creation orientation to the pre-decomposition file so that the 
subsequent run generates the welds in the same way. 
◦  Fix  for  MPP  not  handling  element  deletion  properly  in  some  cases  at  de-
composition boundaries. 
◦  Add new pfile option "contact { keep_acnodes }" which does NOT exclude 
slave  nodes  of  adaptive  constraints  from  contact,  which  is  the  default  be-
havior.  (MPP only.) 
◦  MPP Performance-Related Improvements: 
  Allow user input of *LOAD_SEGMENT_FILE through familied files. 
  Bug fix for *LOAD_SEGMENT_FILE to get correct time history data 
for pressure interpolation. 
  Output two csv files for user to check MPP performance: 
• 
load_profile.csv: general load balance 
•  cont_profile.csv: contact load balance 
  Allow user to control decomp/distribution of multiple airbags using 
*CONTROL_MPP_DECOMPOSITION_ARRANGE_PARTS 
  memory2 = option on *KEYWORD line 
  Disable unreferenced curves after decomposition using *CONTROL_
MPP_DECOMPOSITION_DISABLE_UNREF_CURVES.    This  applies 
to the curves used in the following options to speed up the execution 
several times. 
• 
• 
• 
• 
*BOUNDARY_PRESCRIBED_MOTION_NODE 
*LOAD_NODE 
*LOAD_SHELL_ELEMENT 
*LOAD_THERMAL_VARIABLE_NODE 
◦  Bug fix for *CONTROL_MPP_DECOMPOSITION_SHOW with *AIRBAG_
PARTICLE. 
◦  Fix  cpu  dependent  results  when  using  function  RCFORC()  in  *DEFINE_
CURVE_FUNCTION.  This affects MPP only. 
◦  Fix  hang  up  when  using  *DEFINE_CURVE_FUNCTION  with  element 
function BEAM(id,jflag,comp,rm) and running MPP with np > 1. 
◦  *CONTROL_MPP_DECOMPOSITION:  The  cpu  cost  for  solid  elements  -1 
and -2 are accounted for in the mpp domain decomposition. 
◦  Fix bug in *CONTROL_MPP_IO (Windows platform only) related to insuf-
ficient administrative privileges for writing tmp file on root drive.
◦  Revise  l2a  utility  on  Windows  platform  to  create  identical  node  output 
INTRODUCTION 
format as Linux. 
•  Output 
◦  Fix  for  MPP  external  work  when  bndout  is  output  and  there  are 
*BOUNDARY_PRESCRIBED_MOTION_RIGID commands in the input. 
◦  Fixed  the  output  of  forces  and  associated  energy  due  to  *LOAD_RIGID_
BODY for both explicit and implicit (*DATABASE_BNDOUT). 
◦  Fixed stress and strain output of thick shells when the composite material 
flag  is  set  on  *DATABASE_EXTENT_BINARY.    The  transformation  was 
backwards. 
◦  If the size of a single plot state was larger than the d3plot size defined by 
x=<factor> on the execution line, the d3plot database may not be readable 
by LS-PrePost.  This issue is now fixed. 
◦  *DATABASE_PROFILE:  Output  data  profiles  for  beams  (TYPE = 5)  and 
add density as DATA = 20. 
◦  New  option  HYDRO = 4  on  *DATABASE_EXTENT_BINARY.    Outputs  7 
additional variables: the same 5 as HYDRO = 2 plus volumetric strain (de-
fined  as  Relative  Volume  -  1.0)  and  hourglass  energy  per  unit  initial  vol-
ume. 
◦  Fix  for  binout  output  of  swforc  file  which  can  get  the  data  vs.    ids  out  of 
sync when some solid spotwelds fail. 
◦  Fix for d3plot output of very large data sets in single precision. 
◦  Fix for output of bndout data for joints in MPP, which was writing out in-
correct data in some cases. 
◦  Added  new  option  *INTERFACE_SPRINGBACK_EXCLUDE  to  exclude 
selected portions from the generated dynain file. 
◦  Add a new option to *INTERFACE_COMPONENT_FILE to output only 3 
degrees of freedom to the file, even if the current model has 6. 
◦  Minor  change  to  how  pressure  is  computed  for  triangles  in  the  INTFOR 
output. 
◦  Fix MPP output issue with intfor file. 
◦  Fixes for writing and reading of dynain data in LSDA format. 
◦  Corrected the summation of rigid body moments for output to bndout for 
some special cases in MPP. 
◦  Corrected the output to d3iter when 10 node tets are present (D3ITCTL on 
*CONTROL_IMPLICIT_SOLUTION). 
◦  Enhanced implicit collection of moments for the rcforc file. 
◦  For implicit, convert spc constraint resultant forces to local coordinate sys-
tem for output.  Also corrected Implicit's gathering of resultant forces due 
to certain SPC constraints. 
◦  Fixed the gathering of resultant forces in implicit for prescribed motion on 
nodes of a constrained rigid body for output to bndout.
INTRODUCTION 
◦  Added  output  of  modal  dynamics  modal  variables  to  a  new  file  moddy-
is  controlled  by  *CONTROL_IMPLICIT_MODAL_
  Output 
nout. 
DYNAMICS. 
◦  Corrected the output of resultant forces for Implicit Linear analysis.  Cor-
rected  the output  of resultant  forces  for  MPP  executions.    These  enhance-
ments affect a number of ASCII files including bndout. 
◦  The following 4 enhancements are to the eigensolvers, including that used 
for *CONTROL_IMPLICIT_EIGENVALUE. 
  Standardized  and  enhance  the  warning/error  messages  for  Implicit 
eigensolution for the case where zero eigenmodes are computed and 
returned in eigout and d3eigv. 
  Added nonsymmetric terms to the stiffness matrix for the implicit ro-
tational  dynamics  eigenanalysis.  This  allows  brake  squeal  analysis 
with  the  contact  nonsymmetric  terms  from  mortar  contact  now  in-
cluded in the analysis. 
  Updated implicit eigensolution for problems with unsymmetric stiff-
ness matrices. Fixed Rotational Dynamics eigensolution to work cor-
rectly  when  first  order  matrix  (W)  is  null.  . 
  Added the eigensolution for problems with stiffess (symmetric or un-
symmetric), mass, and damping. 
◦  Improve Implicit's treatment of constrained joints to account for rounding 
to  *CONSTRAINED_JOINT  with  *CONTROL_
  Applicable 
errors. 
IMPLICIT_GENERAL. 
◦  For  implicit  springback,  zero  out  the  forces  being  reported  to  rcforc  for 
those  contact  interfaces  disabled  at  the  time  of  springback.    Also  enhance 
the  removal  of  contact  interfaces  for  springback  computations.    For 
*INTERFACE_SPRINGBACK. 
◦  *DATABASE_RECOVER_NODE is available to recover nodal stress. 
◦  Fix a bug for detailed stress output, eloutdet, for SOLID type 18. 
◦  Support  new  format  of  interface  force  files  for  ALE,  DEM,  and  CPM.  LS-
PrePost can display the correct label for each output component. 
◦  Added *DATABASE_NCFORC_FILTER option to allow the NCFORC data 
to be filtered using either single pass or double pass Butterworth filtering 
to  smooth  the  output. 
  Added  the  same  filtering  capability  to 
*DATABASE_BINARY_D3PLOT.  This capability is specified on the addi-
tional card for the D3PLOT option and does not require "_FILTER" in the 
keyword input. 
◦  Fix  incorrect  mass  properties  for  solids  in  SSSTAT  file  when  using 
*DATABASE_SSSTAT_MASS_PROPERTIES. 
◦  Fix seg fault during writing of dynain file if INSTRN = 1 in *INTERFACE_
SPRINGBACK  and  STRFLG.ne.0  in  *DATABASE_EXTENT_BINARY  and
the 
SPRINGBACK.  Also output warning message, KEY+1104. 
comes 
after 
*INTERFACE_
◦  Fix  zero  strain  values  output 
to  curvout 
for  *DEFINE_CURVE_
FUNCTION using function, ELHIST, for solid elements. 
◦  Fix  missing  parts  in  d3part  when  MSSCL = 1  or  2  in  *DATABASE_
EXTENT_BINARY. 
◦  Fix incorrect damping energy computation for glstat. 
◦  Fix incorrect part mass in d3plot for shells, beams & thick shells. 
◦  Fix  incorrect  curvout  values  when  using  BEAM(id,jflag,comp,rm)  for 
*DEFINE_CURVE_FUNCTION  and  if  the  beam  formulation  is  type  3,  i.e.  
truss. 
◦  Fix incorrect output to curvout file if using ELHIST in *DEFINE_CURVE_
FUNCTION for shells. 
◦  Output stresses for all 4 intg points to eloutdet for cohesive element types 
19 & 20. 
◦  Fix 
incorrect  rotational  displacement  to  nodout  when  REF = 2 
in 
*DATABASE_HISTORY_NODE_LOCAL.  Affects MPP only. 
◦  Fix incorrect strains output to elout for shell type 5 and when NIP > 1. 
◦  Fix  incorrect  acceleration  output  to  nodout  file  when  IACCOP = 1  in 
*ELEMENT_SEATBELT_
IGRAV = 1 
in 
*CONTROL_OUTPUT  and 
ACCELEROMETER. 
◦  Fix  corrupted  d3plot  when  RESPLT = 1 
in  *DATABASE_EXTENT_
BINARY and idrflg.ge.5 in *CONTROL_DYNAMIC_RELAXATION. 
◦  Fix missing element connectivities in nastin file when using *INTERFACE_
SPRINGBACK_NASTRAN_NOTHICKNESS. 
fault  when  using 
seg 
◦  Fix 
*DATABASE_BINARY_D3PART  with 
*CONTACT_TIED_SHELL_EDGE_TO_SURFACE.  This affects SMP only. 
◦  Fix  incorrect  output  to  bndout  when  using  multiple  *LOAD_NODE_
POINT for the same node and running MPP with ncpu > 1. 
◦  Fix incorrect dyna.inc file when using *MAT_FU_CHANG_FOAM/MAT_
83,  *DEFINE_COORDINATE_NODES,  and  *CONSTRAINED_JOINT_
STIFFNESS_GENERALIZED with *INCLUDE_TRANSFORM. 
◦  Fix IEVERP in *DATABASE_EXTENT_D3PART which was not honored in 
writing out d3part files. 
◦  Fix  incorrect  stresses  written  out  to  dynain  for  thick  shells  with  formula-
tions 1,2 and 4. 
◦  Fix incorrect output to disbout data for discrete beams. 
◦  Fix incorrect output to binary format of disbout.  Affects SMP only. 
◦  Fix  error  when  writing  initial  stresses  for  thick  shells  to  dynain.    Affects 
MPP only. 
◦  Fix thick shells strain output to dynain. 
◦  Fix  incorrect  writing  of  material  data  to  dyna.str  for  *MAT_SEATBELT 
when using long = s. 
◦  Fix  coordinate/disp  output  to  d3plot  of  *CONSTRAINED_NODAL_
RIGID_BODY's pnode.
INTRODUCTION 
◦  Fixed  the  initial  d3plot  state  in  SMP  runs  when  tied  contact  is  used  with 
theCNTCO parameter on *CONTROL_SHELL.  The geometry was wrong 
in that state. 
◦  Add cross section forces output (*DATABASE_SECFORC) for cohesive el-
ements ELFORM type 19, 20, 21, and 22. 
◦  Slight increase of precision for values in nodout file. 
◦  Add  new  option  FSPLIT  to  *INTERFACE_SPRINGBACK_LSDYNA  to 
split the dynain file into two files (geometry and initial values). 
◦  *DEFINE_MATERIAL_HISTORIES: New keyword for organizing material 
history outputs, currently only for solids, shells and beams and the d3plot 
output  but  to  be  extended  to  tshells  and  ascii/binout.    The  purpose  is  to 
customize 
that  otherwise  are  output  via 
NEIPS/NEIPH/NEIPB on *DATABASE_EXTENT_BINARY, to avoid vari-
able  conflict  and  large  d3plots  and  thus  facilitate  post-processing  of  these 
variables.    Currently  available  in  small  scale  but  to  be  continuously  ex-
tended. 
the  history  variables 
◦  Fixed  bug  affecting  IBINARY = 1  (32  bit  ieee  format)  in  *DATABASE_
FORMAT.  This option was not working. 
◦  Fixed incorrect printout of node ID for *ELEMENT_INERTIA. 
◦  Increased the header length to 80 for the following files in binout: matsum, 
nodout, spcforc, ncforc 
◦  Fixed bug in which d3msg was not written for SMP. 
◦  The d3plot output for rigid surface contact was incorrect for MPP. 
◦  Fixed bugs when when using curve LCDT to control d3plot output. 
◦  Fixed abnormal increase in  d3plot size  caused by outputting velocity and 
acceleration when data compression is on. 
◦  Added new variable GEOM in *CONTROL_OUTPUT for chosing geome-
try or displacement in d3plot, d3part, and d3drlf. 
◦  Added  command  line  option  "msg="  to  output  warning/error  descrip-
tions.    See  MSGFLG  in  *CONTROL_OUTPUT  for  alternate  method  of  re-
questing such output. Accepted values for "msg=" are message# or all. 
  message#,  e.g.,    KEY+101  or  10101.  This  option  will  print  the  er-
ror/warning message to the screen. 
  all.  this option will print all error/warning messages to d3msg file. 
◦  Fixed bug for *DATABASE_BINARY_D3PROP file if adaptivity used. The 
error caused blank d3prop output. 
◦  *DATABASE_HISTORY_SHELL_SET 
*CONTROL_
ADAPTIVITY caused  error 20211.  The error involves the BOX option be-
ing used for shell history output. 
combined  with 
◦  Added *INTEGRATION...  data to d3prop.
INTRODUCTION 
•  Restarts 
◦  Fix bug when deleted uniform pressure (UP) airbag during simple restart. 
◦  Fix  for  index  error  that  could  cause  problems  for  accelerometers  during 
full deck restart in MPP. 
◦  Fix  for  MPP  output  of  LSDA  interface  linking  file  when  restarting from  a 
dump file. 
◦  Fix incorrect strains in d3plot after restart when STRLG > 1. 
◦  Fix incorrect velocity initialization for SMP full deck restart when using 
◦  *INITIAL_VELOCITY_GENERATION 
*INITIAL_VELOCITY_
and 
GENERATION_START_TIME. 
◦  Fix incorrect behavior of *CONTACT_ENTITY in full deck restart. 
◦  Fix incorrect full deck restart analysis if initial run was implicit and the full 
deck restart run is explicit. 
◦  Fix 
ineffective  boundary  condition 
for  *MAT_RIGID  when  using 
*CHANGE_RIGID_BODY_CONSTRAINT  with  *RIGID_DEFORMABLE_
R2D for small deck restart. 
◦  Fix  initialization  of  velocities  of  *MAT_RIGID_DISCRETE  nodes  after  re-
start using *CHANGE_VELOCITY_GENERATION. 
◦  Fix  internal  energy  oscillation  after  full  deck  restart  when  using 
*CONTACT_TIED_SURFACE_TO_SURFACE_OFFSET with TIEDID = 1 in 
optional card D.  This affects SMP only. 
◦  Corrected  bug  affecting  full  restart  that 
included  any  change  to 
node/element IDs.  This bug has existed since version R6. 
◦  Fixed  bug  affecting  d3plot  times  following  fulldeck  restart  with  curve  in 
SMP. 
◦  Fixed bug in simple restart: *INTERFACE_COMPONENT_FILE forgets the 
filename and writes to infmak instead. 
•  *SENSOR 
◦  Enable full restart for *SENSOR. 
◦  Add optional filter ID to SENSORD of *DEFINE_CURVE_FUNCTION. 
◦  Enable  LOCAL  option  of  *CONSTRAINED_JOINT  to  be  used  with 
*SENSOR_DEFINE_FORCE. 
◦  Fix  a  MPP  bug  that  happens  when  *SENSOR_DEFINE_NODE  has  a  de-
fined N2. 
◦  *SENSOR_CONTROL: 
  Fix a bug for TYPE = JOINTSTIF 
  Fix  a  MPP  bug  for  TYPE = PRESC-MOT  when  the  node  subject  to 
prescribed motion is part of a rigid body 
  Add  TYPE = BELTSLIP  to  control  the  lockup  of  *ELEMENT_
SEATBELT_SLIPRING. 
  Add TYPE = DISC-ELES to delete a set of discrete elements.
INTRODUCTION 
◦  Add FTYPE = CONTACT2D to to *SENSOR_DEFINE_FORCE to track the 
force from *CONTACT_2D. 
◦  Add  the  variable  SETOPT  for  *SENSOR_DEFINE_NODE_SET  and 
*SENSOR_DEFINE_ELEMENT_SET to sense and process data from a node 
set or element set, resp., resulting in a single reported value. 
◦  *SENSOR can be used to control *CONTACT_GUIDED_CABLE. 
◦  Fix  a  bug  related  to  *SENSOR_DEFINE_FUNCTION  triggered  by  more 
than 10 sensor definitions. 
•  SPG (Smooth Particle Galerkin) 
◦  *SECTION_SOLID_SPG 
(KERNEL = 1):  The  dilation  parameters 
(DX,DY,DZ)  of  SPG  Eulerian  kernel  are  automatically  adjusted  according 
to the local material deformation to prevent tensile instability. 
•  SPH (Smooth Particle Hydrodynamics) 
◦  Retain user IDs of SPH particles in order to ensure consistent results when 
changing the order of include files. 
◦  Add feature to inject SPH particles, *DEFINE_SPH_INJECTION. 
◦  Added support of various material models for 2D and 3D SPH particles: 
  *MAT_098 (*MAT_SIMPLIFIED_JOHNSON_COOK) 
  *MAT_181 (*MAT_SIMPLIFIED_RUBBER) 
  *MAT_275 (*MAT_SMOOTH_VISCOELASTIC_VISCOPLASTIC) 
◦  Added support of *DEFINE_ADAPTIVE_SOLID_TO_SPH for 2D shell el-
ements and 2D axisymmetric shell elements. 
◦  When using *DEFINE_ADAPTIVE_SOLID_TO_SPH, eliminated duplicate 
kinetic energy calculation for SPH hybrid elements (both SPH particles and 
solid elements contributed kinetic energy into global kinetic energy). 
◦  Added  support  of  second  order  stress  update  (OSU = 1  in  *CONTROL_
ACCURACY keyword) for 2D and 3D SPH particles.  This is necessary for 
simulation of spinning parts. 
◦  Added  ISYMP  option  in  *CONTROL_SPH  to  define  as  a  percentage  of 
original  SPH  particles  the  amount  of  memory  allocated  for  generation  of 
SPH ghost nodes used in *BOUNDARY_SPH_SYMMETRY_PLANE. 
◦  Fixed unsupported part and part set option in *BOUNDARY_SPH_FLOW. 
◦  Fixed unsupported ICONT option from *CONTROL_SPH when combined 
with *BOUNDARY_SPH_FLOW. 
◦  *DEFINE_SPH_TO_SPH_COUPLING:  Output  contact  forces  between  two 
SPH parts (x,y,z and resultant forces) into sphout. The forces can be plotted 
by LS-PrePost. 
◦  *CONTACT_2D_NODE_TO_SOLID:  Added  bucket  sort  searching  algo-
rithm to speed up the process of finding contact pairs between SPH parti-
cles and solid segments.
INTRODUCTION 
•  Thermal 
◦  Corrected a long standing bug in MPP thermal associated with spotwelds 
(*CONSTRAINED_SPOTWELD)  using  thermal  linear  solver  option  11  or 
greater.  The spotweld loads were not being loaded correctly due to an in-
dexing issue in MPP. 
◦  Fix for thermal with *CASE. 
◦  Fix MPP support for thermal friction in SOFT = 4 contact. 
◦  Fixed bug where thermal solver gives a non-zero residual even though no 
loads are present. 
◦  Added  SOLVER = 17 
(GMRES  solver) 
to  *CONTROL_THERMAL_
SOLVER for the conjugate heat transfer problem.  The GMRES solver has 
been  developed  as  an  alternative  to  the  direct  solvers  in  cases  where  the 
structural thermal problem is coupled with the fluid thermal problem in a 
monolithic approach using the ICFD solver.  A significant savings of calcu-
lation time can be observed when the problem reaches 1M elements.  This 
solver is implemented for both SMP and MPP. 
◦  *CONTACT_(option)_THERMAL 
(3D  contact  only):  Add  variable 
FRTOHT to specify fraction of frictional energy applied to slave surface.  It 
follows that  1.-FRTOHT is applied to master surface.  Default is 0.5 which 
gives a 50% - 50% split between the slave and master surfaces which was 
hardwired in prior releases. 
◦  First  release  of  AUTOMATIC_SURFACE_TO_SURFACE_TIED_WELD_
THERMAL. 
  This  will  only  work  when  used  with  BOUNDARY_
THERMAL_WELD.    This  combination  of  keywords  will  activate  a  condi-
tion where sliding contact will become tied contact on cooldown when the 
temperature  of  the  segments  in  contact  go  above  an  input  specified  tem-
perature limit during welding. 
◦  *LOAD_THERMAL_D3PLOT: The d3plot data base was changed such that 
the 1st family member contains control words, geometry, and other control 
entities.  Time state data begins in the 2nd family member.  This change al-
lows the new d3plot data structure to be read in by LS-DYNA when using 
the  *LOAD_THERMAL_D3PLOT  keyword.  This  change  is  not  backward 
compatible.  The old d3plot data structure will no longer be read correctly 
by LS-DYNA. 
◦  Synchronize data in TPRINT for SMP and MPP: 
  Fixed output to tprint/binout for thermal contact. 
  Fixed part IDs for part energies. 
  Fixed format of TPRINT file generated by l2a. 
◦  Fixed handling of start time defined with *CONTROL_START for thermal 
solver. 
◦  Change  the  maximum  number  of  *LOAD_HEAT_CONTROLLER  defini-
tions from 10 to 20.
INTRODUCTION 
◦  Added a third parameter to the TIED_WELD contact option.  The parame-
ter  specifies  heat  transfer  coefficient  h_contweld  for  the  welded  contact.  
Before welding, the parameter from the standard card of the thermal con-
tact is used. 
◦  Parameter FRCENG supported for mortar contact to yield heat in coupled 
thermomechanical problems. 
•  XFEM (eXtended Finite Element Method) 
◦  Added ductile failure to XFEM using critical effective plastic strain as fail-
ure criterion. 
•  Miscellaneous 
◦  Support *SET_NODE_GENERAL PART with SPH and DES. 
◦  *DEFINE_POROUS_...:  Compute  the  coefficients  A  and  B  with  a  user  de-
fined routine in dyn21.F. 
bugs 
◦  Fixed 
in 
Staged 
Construction 
(*DEFINE_STAGED_
CONSTRUCTION_PART): 
  Staged  construction  not  working  on SMP  parallel.    Symptoms  could 
include wrong elements being deleted. 
  Staged construction with beam elements of ELFORM = 2: when these 
beams are dormant, they could still control the time step. 
  Staged  construction  with  *PART_COMPOSITE.    The  bug  occurred 
when  different  material  types  were  used  for  different  layers  within 
the same part, and that part becomes active during the analysis.  The 
symptom of the bug was that stresses and/or history variables were 
not set to zero when the part becomes active. 
◦  Bugs fixed in *DAMPING_FREQUENCY_RANGE_DEFORM:  
  Incorrect results when large rigid body rotations occur. 
  If  RYLEN  on  *CONTROL_ENERGY = 2,  the  energy  associated  with 
this damping should be included in the Internal Energy for the rele-
vant part(s).  This energy was being calculated only if there was also 
*DAMPING_PART_STIFFNESS in the model.  Now fixed - the damp-
ing  energy  will  be  included  in  the  internal  energy  whenever 
RYLEN = 2. 
◦  Fixed NID option of *DEFINE_COORDINATE_VECTOR (bug occurred in 
MPP only). 
◦  Fix lsda open mode to require only minimal permissions to avoid unneces-
sary errors, for example if using an interface linking file that is read only. 
◦  Fix  for  DPART  processing  (*SET_..._GENERAL)  for  solid  and  thick  shell 
elements.
INTRODUCTION 
◦  Fix for JOBID > 63 characters. 
◦  Fix  input  processing  problem  (hang)  that  could  happen  in  some  unusual 
cases if encrypted *INCLUDE files are used. 
◦  Fix interaction of *CASE with jobid = on command line, so the jobid on the 
command line is combined with the generated case ids instead of being ig-
nored. 
◦  *INCLUDE_NASTRAN: 
  Integration defaults to Lobatto for Nastran translator. 
  The default number of integration points is set to 5 for Nastran trans-
lator. 
◦  Issue 
error  message 
TRANSFORMATION is specified. 
and 
terminate  when 
illegal 
*DEFINE_
◦  Add OPTION = POS6N to *DEFINE_TRANSFORMATION to define trans-
formation with 3 reference nodes and 3 target nodes. 
◦  Add OPTION = MIRROR to *DEFINE_TRANSFORMATION. 
◦  Fix a bug that could occur when adapted elements are defined in a file in-
cluded by *INCLUDE_TRANSFORM. 
◦  Fix  a  bug  that  could  occur  when  *BOUNDARY_SPC_SYMMETRIC_
PLANE is used together with *INCLUDE_TRANSFORM. 
◦  Fix  a  bug  that  occurs  when  *DEFINE_BOX  is  included  by  *INCLUDE_
TRANSFORM. 
◦  Make *SET_NODE_COLLECT work together with *NODE_SET_MERGE. 
◦  Fix incorrect shell set generated when using *SET_SHELL_GENERAL with 
OPTION = PART. 
◦  Add  error  trap  for  *SET_PART_LIST_GENERATE_COLLECT  to  catch 
missing part IDs. 
◦  Fixed bug in *INCLUDE_TRANSFORM for adaptive case if JOBID is used. 
◦  Fixed  bug  in  memory  allocation  for  *DEFINE_CURVE  if  total  number
of  points  in 
curve is more than 100. 
◦  Fixed bug with *INCLUDE_TRANSFORM and *CONTROL_ADAPTIVITY 
due  to  an  *INCLUDE  inside  *INCLUDE_TRANSFORM  file.    Added  new 
  The  *NODE, 
files:  adapt.inc# 
*ELEMENT_SHELL  and  *ELEMENT_SOLID  are  removed  from  include 
file. 
for  *INCLUDE_TRANSFORM 
file. 
◦  Fixed bug for DPART option in *SET_SEGMENT_GENERAL.  DPART op-
tion was treated as PART option before. 
◦  Fixed failure of *PARAMETER definition in long format. 
◦  Fixed error in reading solid id for *SET_SOLID_GENERAL. 
◦  Ignore any nonexistant part set IDs in *SET_PART_ADD. 
◦  Fix bug in which sense switches sw2 and sw4 don't work when the output 
interval for glstat is small. 
◦  Fixed bug if *DEFINE_CURVE is used to define adaptivity level.
INTRODUCTION 
◦  Three new keywords are implemented in support of user defined subrou-
tines: *MODULE_PATH[_RELATIVE], MODULE_LOAD, MODULE_USE. 
  The  MODULE  feature  allows  users  to  compile  user  subroutines  into 
dynamic libraries without linking to the LS-DYNA main executable. 
  The dynamic libraries are independent from the main executable and 
do not need to be recompiled or linked if the main executable is up-
dated. 
  This feature loads multiple dynamic libraries on demand as specified 
in the keywords. 
  Without  the  MODULE  feature,  only  one  version  of  each  umat  (such 
as  umat41)  can  be  implemented.    With  the  MODULE  feature,  most 
umat subroutines can be have multiple versions in multiple dynamic 
libraries, and used simultaneously. 
  The MODULE feature supports all user subroutines. 
  The  LS-DYNA  main  executable  may  also  run  without  any  dynamic 
libraries if no user subroutines are required. 
Capabilities added to create LS-DYNA R10.0:  
See release notes (published separately) for further details. 
•  *AIRBAG 
◦  Enhance the robustness of *AIRBAG_INTERACTION to help avoid insta-
bility in MPP when the interaction involves more than two bags. 
◦  *AIRBAG_PARTICLE: 
  Adjust dm_out calculation of vent hole to avoid truncation error. 
  Fix bug in chamber output when there are multiple airbags and mul-
tiple chambers not in sequential order. 
  Bug fix for closed volume of airbag/chamber with intersecting tubes. 
  Add new feature to allow user to define local coordinates of jetting of 
particles through internal vents. 
  Support *SENSOR_CONTROL for CPM airbag. 
  CPM  is  not  supported  for  dynamic  relaxation.    Disable  CPM  airbag 
feature during DR and reactivate airbag following DR. 
  Allow solid parts in definition of internal part set.  The solid volume 
will be excluded from the airbag volume. 
  Allow  additional  internal  part  set  for  shells.    The  shell  part  should 
form  a  closed volume and  its  volume  will  be  excluded  from the  air-
bag volume. 
•  *ALE
INTRODUCTION 
◦  *LOAD_BLAST_SEGMENT:  Automatically  generate  the  ALE  ambient  el-
ements attached to a segment or segment set. 
◦  *BOUNDARY_AMBIENT_EOS: 
implement 
*DEFINE_CURVE_FUNCTION  for  the  internal  energy  and  relative  vol-
ume curves. 
◦  *CONTROL_ALE, 
*CONSTRAINED_LAGRANGE_IN_SOLID 
and 
*ALE_REFERENCE_SYSTEM:  If  NBKT < 0 
in  *CONTROL_ALE,  call 
*DEFINE_CURVE  to  load  a  curve  defining  the  number  of  cycles  between 
bucket sorting in function of time.  If NBKT > 0, the bucket sorting is acti-
vated if the mesh rotations and deformations are large. 
◦  *ALE_FSI_TO_LOAD_NODE:  Implement  a  mapping  of  the  FSI  accelera-
tions 
by 
forces/masses) 
*CONSTRAINED_LAGRANGE_IN_SOLID  (ctype = 4)  between  different 
meshes. 
computed 
(penalty 
◦  DATABASE_FSI, 
and 
*DATABASE_BINARY_FSILNK: Add a parameter CID to output fsi forces 
in a local coordinate system. 
◦  Structured ALE (S-ALE) solver: 
*DATABASE_BINARY_FSIFOR 
  ALE  models  using  rectilinear  mesh  can  be  directly  converted  to  S-
ALE models and run using S-ALE solver by assigning CPIDX = -1 in 
*ALE_STRUCTURED_MESH. 
  S-ALE 
via 
*ALE_STRUCTURED_MESH_CONTROL_POINTS. 
progressive  mesh 
generation 
RATIO 
in 
◦  Recode  ALE  Donor  Cell/Van  Leer  advection  routines  and  restructure 
communication  algorithm. 
*CONSTRAINED_LAGRANGE_IN_SOLID 
These give 30% improvement in run time. 
•  *BOUNDARY 
◦  *BOUNDARY_PWP  can  now  accept  a  *DEFINE_FUNCTION  instead  of  a 
load  curve.  The  input  arguments  are  the  same  as  for  *LOAD_SEGMENT: 
(time, x, y, z, x0, y0, z0). 
option 
for 
of 
*BOUNDARY_PRESCRIBED_ORIENTATION_RIGID  to  offset  the  curves 
by the birth time. 
"toffset" 
◦  Add 
◦  MPP now supports MCOL coupling, *BOUNDARY_MCOL. 
◦  Fix  bug  of  there  being  fully  constrained  motion  of  a  rigid  part  when  pre-
with 
one 
in 
scribing 
translational 
*BOUNDARY_PRESCRIBED_MOTION_RIGID  while 
*MAT_RIGID, i.e., all rotational dof are constrained. 
dof 
con2 = 7 
more 
than 
◦  Instead  of  error  terminating  with  warning  message,  STR+1371,  when 
*BOUNDARY_PRESCRIBED_MOTION and *BOUNDARY_SPC is applied
INTRODUCTION 
to same node and dof, issue warning message, KEY+1106, and release the 
conflicting SPC. 
erroneous 
SET_BOX 
results 
option 
used 
for 
is 
if 
◦  Fix 
*BOUNDARY_PRESCRIBED_MOTION. 
◦  Fix  *BOUNDARY_PRESCRIBED_ACCELEROMETER_RIGID  for  MPP.    It 
may  error  terminate  or  give  wrong  results  if  more  than  one  of  this  key-
word is used. 
◦  Fix 
segmentation 
using 
*BOUNDARY_PRESCRIBED_ORIENTATION  with  vad = 2,  i.e.    cubic 
spline interpolation. 
when 
fault 
◦  Added  instruction  *BOUNDARY_ACOUSTIC_IMPEDANCE  for  explicit 
calculations that applies an impedance boundary condition to the bounda-
ry of *MAT_ACOUSTIC element faces.  This is a generalization of the non-
and 
reflecting 
*BOUNDARY_ACOUSTIC_IMPEDANCE may be used on the same faces, 
in which case the boundary acts like both and entrant and exit boundary. 
◦  Fixed a problem with non-reflecting boundaries redefining the bulk modu-
condition. 
boundary 
*LOAD 
Both 
lus which caused contact to change behavior. 
◦  Added support for acoustic materials ith non-reflective boundaries. 
◦  Fix the single precision version so that *INCLUDE_UNITCELL now has no 
problem to identify pairs of nodes in periodic boundaries. 
◦  When  using  *INCLUDE_UNITCELL  to  generate  Periodic  Boundary  Con-
straints (PBC) for an existing mesh, a new include file with PBCs is gener-
ated instead of changing the original mesh input file.  For example, if users 
include a file named "mesh.k" through *INCLUDE_UNITCELL (INPT = 0), 
a new include file named "uc_mesh.k" is generated where all PBCs are de-
fined automatically following the original model information in mesh.k. 
◦  *INCLUDE_UNITCELL  now  supports  long  input  format  in  defining  the 
element IDs. 
◦  Include SPC boundary conditions as part of H8TOH20 solid element con-
version. 
◦  Add  a  new  option  SET_LINE  to  *BOUNDARY_PRESCRIBED_MOTION: 
This option allows a node set to be generated including existing nodes and 
new  nodes  created  from  h-adaptive  mesh  refinement  along  the  straight 
line connecting two specified nodes to be included in prescribed boundary 
conditions. 
•  BLAST 
◦  *PARTICLE_BLAST and DES: 
  Consider eroding of shell and solid in particle_blast. 
  Support interface force file output for gas particle-structure coupling. 
  Bug fix for wet DES coupled with beam. 
  Support *SET_NODE_GENERAL PART with SPH or DES.
INTRODUCTION 
  MPP  now  uses  async  communication  for  DES  coupling  to  improve 
general performance. 
  Support  for  solid  element  when  modeling  irregular  shaped  charge 
with HECTYPE = 0/1 in *PARTICLE_BLAST. 
  Output adaptive generated DES and NODE to a keyword file. 
◦  Fix  inadvertent  detonation  of  HE  part  when  there  are  more  than  one  HE 
is  not  defined  with 
the  HE  part 
though 
even 
part  and 
*INITIAL_DETONATION. 
explicit 
to 
explicit 
◦  Fixed 
*BOUNDARY_USA_COUPLING 
support 
*INITIAL_STRESS and *INITIAL_STRAIN_ usage, typically from a dynain 
file. 
◦  Fixed 
support 
*CONTROL_DYNAMIC_RELAXATION  IDRFLF = 5,  so  a  static  implicit 
calculation can be used to initialize/preload a model before conducting an 
explicit  transient  calculation.    If  inertia  relief  is  used  during  the  static 
phase, 
with 
*CONTROL_IMPLICIT_INERTIA_RELIEF for the explilcit phase. 
*BOUNDARY_USA_COUPLING 
disabled 
must 
then 
be 
to 
it 
◦  Support  imperial  unit  system  for  *PARTICLE_BLAST.  mass = lbf-s2/in, 
length = inch, time = second, force = lbf, pressure = psi. 
◦  Add  option 
to  define  detonation  point  using  a  node 
for 
*PARTICLE_BLAST.  
◦  Add  interface  force  file  output  for  *PARTICLE_BLAST  with  keyword 
*DATABASE_BINARY_PBMFOR  and  command  line  option  "pbm=".  This 
output of forces for gas-particle-structure coupling. 
◦  For *PARTICLE_BLAST, add built-in smoothing function for particle struc-
ture interaction. 
◦  For  *PARTICLE_BLAST,  when  coupling  with  DEM,  the  DEM  nodes  that 
are inside HE domain are automatically deactivated. 
◦  Add  support  for  solid  elements  when  modeling  irregular  shaped  charge 
with HECTYPE = 0/1 for *PARTICLE_BLAST.  The original approach only 
supports  shell  elements  and  the  initial  coordinates  of  HE  particle  are  at 
shell surface.  The model had to relax several hundred time step to let par-
ticle  fill  in  the  interior  space,  which  was  not  convenient.    Using  new  ap-
proach, the initial positions of HE particles are randomly distributed inside 
the container by using solid element geometry.  Both hex and Tet solids are 
supported. 
◦  For particle blast method (PBM), consider reflecting plane as infinite. 
◦  Change 
the  name  of  keyword  *DEFINE_PBLAST_GEOMETRY 
to 
*DEFINE_PBLAST_HEGEO. 
•  *CESE (Compressible Fluid Solver) 
◦  CESE time steps:
INTRODUCTION 
  Modified  the  blast  wave  boundary  condition  treatment  to  make  it 
(with 
calculations 
stable 
wave 
more 
blast 
*LOAD_BLAST_ENHANCED). 
in 
  The flow field calculation will be skipped if the structural time-step is 
much smaller than the fluid time step, until both time-steps reach the 
same order.  This will save CPU time in some fluid/structure interac-
tion (FSI) problem calculations. 
  In addition to depending upon the local CFL number, the fluid time 
step  'dt'  calculation  has  been  modified  to  also  adjust  dynamically  to 
extreme flow conditions.  This makes stiff flow problems more stable 
especially in 3D fluid problem calculations when the mesh quality is 
poor. 
◦  Moving mesh solvers: 
  Corrected  several  aspects  of  the  implicit  ball-vertex  (BV)  mesh  mo-
tion solver for the following keywords:  
*ICFD_CONTROL_MESH_MOV 
*CESE_CONTROL_MESH_MOV. 
  The absolute tolerance argument is no longer used by the BV solver.  
As  an  example,  the  following  is  all  that  is  needed  for  CESE  moving 
mesh problems:  
*CESE_CONTROL_MESH_MOV 
  $     ialg   numiter    reltol 
             1            500   1.0e-4 
  Also  corrected  the  CESE  moving  mesh  solvers  for  a  special  case  in-
volving a wedge element.  Also, fixed the d3plot output of wedge el-
ement connectivities for the CESE moving mesh solvers. 
◦  CESE d3plot output: 
  Added  real  2D  CESE  output,  and  this  is  confirmed  to  work  with 
LSPP4.3  and  later  versions.    This  also  works  for  d3plot  output  with 
the 2D CESE axisymmetric solver. 
  For  all  immersed-boundary  CESE  solvers,  corrected  the  plotting  of 
the Schlieren number and the chemical species mass fractions. 
  The  following  new  CESE  input  cards  are  related  to  surface  d3plot 
output: 
*CESE_SURFACE_MECHSSID_D3PLOT 
*CESE_SURFACE_MECHVARS_D3PLOT 
In  conjunction  with  the  above,  new  FSI  and  conjugate  heat  transfer 
output on solid (volume) mesh outside boundaries is now supported. 
◦  CESE immersed-boundary method (IBM) FSI solvers:
INTRODUCTION 
  *CESE_FSI_EXCLUDE  is  a  new  keyword  for  use  with  the  CESE  im-
mersed boundary method FSI solvers.  With it, unnecessary structur-
al parts that are not actively participating in the FSI in the CESE IBM-
FSI solver can now be excluded from the CESE FSI calculation.  This 
is  also  supported  for the  case  when  some  of  the  mechanics  parts  in-
volve element erosion. 
◦  CESE chemistry solvers: 
  In R10, we also updated several things in the FSI solver with chemis-
try called FSIC. In chemical reacting flow, a delta time between itera-
tions  is  extremely  important  for  code  stabilization  and  thus,  to  get 
reasonable results.  To this end, we optimized such an iterative delta 
time, which is based on the CFL number.  This optimization is based 
on  the  gradient  of  the  local  pressure,  which  we  think  will  dominate 
control of the CFL number. 
  Next,  the  total  number  of  species  are  increased  up  to  60  species  in 
chemical  reacting  flow, so  that the  reduced  Ethylene  (24~53  species) 
and  Methane  (20~60  species)  combustion  are  possible  with  this  ver-
sion.  
  We will update more practical examples about FSIC problems includ-
ing precise experimental validations. 
  Note that we can provide some related examples upon user request. 
  Other corrections of note include the following: 
Brought  in  enthalpy-related  corrections  to  the  CESE  chemistry  solv-
ers. 
Fixed the conjugate heat transfer boundary condition for the 2D and 
3D CESE fixed mesh chemistry solvers. 
Corrected the initialization of fluid pressure for CESE IBM chemistry 
solvers. 
Enabled  output  of  the  timing  information  for  the  CESE  chemistry 
solvers. 
Added restart capability to the CESE chemistry solvers. 
•  *CHEMISTRY 
◦  New  inflator  models  of  Pyrotechnic  and  Hybrid  type  are  updated.    It  is 
important to note that these are basically 0-dimensional models via the fol-
lowing two main keywords, 
*CHEMISTRY CONTROL_INFLATOR 
*CHEMISTRY_INFLATOR_PROPERTIES 
◦  By using the *CHEMISTRY CONTROL_INFLATOR keyword, the user can 
select the type of the solver, output mode, running time, delta t, and time 
interval for output of time history data.  
For example, if we have a keyword set up as,
INTRODUCTION 
*CHEMISTRY CONTROL_INFLATOR, 
  $  isolver   ioutput   runtime      delt    p_time 
                     1              0            0.1   1.0e-6      5.0e-4 
with "isolver set to 1", the user can simulate a conventional Pyrotechnic in-
flator mode, while with "isolver" set to 2 or 3, Hybrid inflator simulation is 
possible. 
◦  In addition, to continue an airbag simulation via an ALE or CPM method, 
the user can save the corresponding input data file by using "ioutput" op-
tion.  For more details about airbag simulations using a saved data file, re-
fer to the keyword manual. 
◦  Also, note that the updated version has two options for the Hybrid models: 
  isolver = 2 => Hybrid model for the cold flow 
  isolver = 3 => Hybrid model for the heated flow. 
◦  In the *CHEMISTRY_INFLATOR_PROPERTIES keyword, there are sever-
al  cards  to  set  up  the  required  properties  of  an  inflator  model.    The  first 
two cards are for the propellant properties involved in inflator combustion. 
For example, 
  $card1: propellants 
  $  comp_id     p_dia  p_height    p_mass   p_tmass 
                 10       0.003      0.0013        2.0e-5   5.425e-3 
  $card2: control parameters 
  $  t_flame    pindex        A0     trise    rconst 
           2473.          0.4  4.45e-5       0.0      0.037 
In the first card, the user can specify the total amount of propellant parti-
cles and their shape. 
Using the second card, the user can also specify the thermodynamics of the 
propellant and its burning rate.  
To support the options in card2, especially the second option, pindex, and 
the third, A0, we provide a standalone program upon request for the pro-
pellant equilibrium simulation. 
The  remaining  cards  are  for  the  combustion  chamber,  gas  chamber,  and 
airbag, respectively. 
•  *CONTACT 
◦  *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_MORTAR_TIED_
WELD for modeling welding has been added.  Surfaces are tied based on 
meeting  temperature  and  proximity  criteria.    Non-MORTAR  version  of 
this contact was introduced at R9.0.1. 
◦  Fix issue setting contact thickness for rigid shells in ERODING contact. 
◦  Add  MPP  support  for  *CONTACT_AUTOMATIC_GENERAL  with  adap-
tivity.
INTRODUCTION 
◦  Change  "Interface  Pressure"  report  in  intfor file  from  abs  (force/area)  to  -
force/area,  which  gives  the  proper  sign  in  case  of  a  tied  interface  in  ten-
sion. 
◦  Rework  input  processing  so  that  more  than  one  *CONTACT_INTERIOR 
may be used, and there can be multiple part sets in each one. 
◦  Minor change to how pressure is computed for triangles in the intfor data-
base. 
◦  Fix 2 bugs for contact involving high order shell elements: 
-  When high order shell elements are generated by SHL4_TO_SHL8. 
-  When using a large part id like 100000001. 
◦  Implement  a  split-pinball  based  contact  option  for  neighbor  elements  in 
segment-based  contact.    Invoke  this  option  by  setting  |SFNBR|>=1000.  
The new algorithm is more compatible with DEPTH = 45 so that there is no 
longer a need to split quads. 
◦  The  effect  of  shell  reference  system  offsets  on  contact  surface  location  is 
now  properly  considered  when  running  MPP.    The  shell  offset  may  be 
specified using NLOC in *SECTION_SHELL or in *PART_COMPOSITE, or 
by using the OFFSET option of *ELEMENT_SHELL. This effect on contact 
is only considered when CNTCO is set to 1 or 2 in *CONTROL_SHELL. 
◦  Fix 
of 
bug 
for 
*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE  after  dynamic  re-
laxation when consistency is on in SMP. 
time = 0.0 
forces 
rcforc 
zero 
in 
at 
◦  Fix  input  error  when  using  many  *RIGIDWALL_GEOMETRIC_...    with 
_DISPLAY option. 
◦  Fix input error when *CONTACT_ENTITY is attached to a beam part, PID. 
◦  Fix  error  termination  due  to  negative  volume,  SOL+509,  even  when 
*CONTACT_ERODING...  is set.  This affects MPP only. 
◦  Check whether a slave/master node belongs to a shell before updating the 
nodal 
*CONTROL_SHELL  and 
SST/MST.ne.0.0  and  in  SSFT/SMFT = 0.0  card  3  of  *CONTACT_.....    For 
SMP only. 
thickness  when 
ISTUPD > 0.0 
in 
◦  Fix 
penetrating 
nodes 
when 
◦  Fix 
*CONTACT_ERODING_NODES_TO_SURFACE  with 
*MAT_142/*MAT_ 
seg 
using 
*CONTACT_AUTOMATIC_SINGLE_SURFACE_TIED  with  consistency 
mode, .i.e.  ncpu < 0, for SMP. 
when 
fault 
SOFT = 1 
using 
in 
◦  Fix 
corrupted 
intfor  when 
using 
parts/part 
sets 
in 
*CONTACT_AUTOMATIC_....This affects SMP only. 
◦  Implement  incremental  update  of  normal  option,  invoked  by  TIEDID = 1, 
for  *CONTACT_TIED_NODES_TO_SURFACE_CONSTRAINED_OFFSET 
for SMP. 
◦  Fix 
unconstrained 
nodes 
when 
using 
*CONTACT_TIED_SURFACE_TO_SURFACE_CONSTRAINED_OFFSET 
resulting in warning message, SOL+540.  This affects SMP only.
INTRODUCTION 
◦  Fix 
spurious 
repositioning 
of 
nodes 
when 
using 
*CONTACT_SURFACE_TO_SURFACE for SMP. 
◦  Added support to segment based contact for the SRNDE parameter on op-
tional card E.  This option allows round edge extensions that do not extend 
beyond  shell  edges  and  also  square  edges.    The  latter  overlaps  with  the 
SHLEDG parameter on card D. 
◦  Fixed  a  potential  memory  error  that  could  occur  during  segment  based 
contact input. 
◦  Fixed an error that could cause an MPP job to hang in phase 3.  The error 
could  occur  when  SOFT = 2  contact  is  used  with  the  periodic  intersection 
check and process 0 does not participate in the contact. 
◦  Modified SOFT = 2 contact friction when used with *PART_CONTACT to 
define friction coefficients, and the two parts in contact have different coef-
ficient values.  With this change, the mu values used for contact will be the 
average of the values that are calculated for each part.  Prior to this change, 
mu was calculated for only the part that is judged to be the master.  This 
change makes the behavior more predictable and also makes it behave like 
the other contacts with SOFT = 0 and SOFT = 1. 
◦  Fixed 
◦  Added  a  warning  message  (STR+1392)  for  when  trying  to  use  the  OR-
THO_FRICTION contact option with SOFT = 2 contact, because that option 
is not available.  The contact type is switched to SOFT = 1. 
in 
MPP 
*CONTACT_2D_AUTOMATIC_SURFACE_TO_SURFACE  when  used 
with node sets to define the contact surfaces.  The master side was likely to 
trigger a spurious error about missing nodes that terminated the job. 
serious 
error 
file 
not 
force 
could 
support  NFAIL = 1 
◦  Switched segment based (SOFT = 2) non-eroding contact to prevent it from 
adding  any  new  segments  when  brick  element  faces  are  exposed  when 
other elements are deleted.  There were two problems.  The first is that the 
interface 
on 
*DATABASE_EXTENT_INTFOR  because  the  intfor  file  does  not  expect 
new segments to replace the old, so it  just  undeletes the old segments in-
stead  of  adding  the  new.    The  second  problem  is  that  when  non-eroding 
contact  is  used,  we  only  have  enough  memory  in  fixed  length  arrays  for 
the  segments  that  exist  at  t = 0.    When  segments  are  deleted,  I  was  using 
the space that they vacated to create new segments, but it was very likely 
that some segments could not be created when the number of open spaces 
was  less  than  the  number  of  new  segments  that  are  needed.    In this  case, 
some  segments  would  not  be  created  and  there  would  be  surfaces  that 
could  be  penetrated  with  no  resistance.    This  behavior  is  impossible  to 
predict, so it seems better to prevent any new segments from being created 
unless eroding contact is used. 
◦  Fixed rcforc output for MPP 2D automatic contact.  The forces across pro-
cessors were missed.
INTRODUCTION 
◦  Fixed a segment based contact error in checking airbag segments.  This af-
fects  only  airbags  that  are  defined  by  control  volumes,  that  is  defined  by 
*AIRBAG.  The symptom was a segmentation fault. 
◦  Fixed SMP eroding segment based (SOFT = 2) contact which was not acti-
vating the negative volume checking of brick elements.  The MPP contact 
and the other SMP contacts were doing this but not SMP SOFT = 2. 
◦  Fixed  support  for  CNTCO  on  *CONTROL_SHELL  by  segment  based 
(SOFT = 2) contact.  It was adjusting the contact surface only half of what it 
should have done. 
◦  Fixed  eroding  segment  based  contact  when  used  with  the  CNTCO > 0  on 
*CONTROL_CONTACT.  A segmentation fault was occurring. 
◦  Modified  MPP  segment  based  (soft = 2)  contact  to  use  R8  buffers  to  pass 
nodal  coordinates.    This  should  reduce  MPP  scatter  when  decomposition 
changes. 
◦  Added support for using a box to limit the  contact segments to those ini-
tially in the box when using eroding segment based contact.  The box op-
tion  has  not  been  available  for  any  eroding  contact  up  until  now.  
(SOFT = 2 and SBOXID, MBOXID on *CONTACT_ERODING_...). 
◦  Fixed  force  transducers  with  MPP  segment  based  contact  when  segments 
are involved with multiple, 2-surface force transducers.  The symptom was 
that  some  forces  were  missed  for  contact  between  segments  on  different 
partitions. 
◦  Added support for *ELEMENT_SOURCE_SINK used with segment based 
contact.  With this update, inactive elements are no longer checked for con-
tact. 
◦  Fixed an MPP problem in segment based contact that cased a divide by ze-
ro during the bucket sort.  During an iteration of the bucket sort, all active 
segments were somehow in one plane which was far from the origin such 
that a dimension rounded to zero.  The fix for this should affect only this 
rare case and have no effect on most models. 
◦  Modified segment based (SOFT = 2) contact to make SMP and hybrid fast-
er, particularly for larger numbers of processors. 
◦  Fixed thermal MPP segment based contact.  The message passing  of ther-
mal  energy  due  to  friction  was  being  skipped  unless  peak  force  data  was 
written to the intfor file. 
◦  Fixed  likely  memory  errors  in  MPP  problems  with  2D  automatic  contact 
when friction is used. 
◦  Support  the  VC  parameter  (coefficient  for  viscous  friction)  in  the  case  of 
segment based contact, which has previously been unsupported.  This op-
tion  will  work  best  with  FNLSCL > 0,  DNLSCL = 0  on  optional  card  D.  
The card D option causes the contact force to be proportional to the over-
lap area which causes even pressure distribution. 
◦  Enabled segment based contact (SMP and MPP) to work with type 24 (27-
node) brick elements.
INTRODUCTION 
◦  Fixed  MPP  segment  based  contact  for  implicit  solutions.    During  a  line 
search, some data was not restored correctly when the solver goes back to 
the last converged state.  This caused possible memory errors. 
◦  Fixed  friction  for  MPP  segment  based  contact  in  the  implicit  solver.    The 
sliding  velocity  was  calculated  incorrectly  using  the  explicit  time  step  ra-
ther than the implicit step. 
◦  Fixed  a  bug  in  MPP  *CONTACT_2D_AUTOMATIC...,  where  a  flaw  in 
code used during MPP initialization could cause segments to fail to detect 
penetration. 
◦  Fixed 
the 
of 
*CONTACT_2D_AUTOMATIC_SINGLE_SURFACE  in  the  MPP  version.  
There  was  a  memory  error  that  could  occur  if  thick  beams  were  in  the 
model. 
checking 
beam 
thick 
◦  New 
values 
history 
(*USER_INTERFACE_FRICTION):  material  directions,  relative  velocity 
components and yield stress. 
element 
friction 
user 
for 
◦  Add  new  user-defined 
interface  for  tiebreak  contact 
invoked  by 
*CONTACT_AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE_TIEB
REAK_USER. 
◦  MORTAR CONTACT 
  PENMAX  and  SLDTHK  has  taken  over  the  meanings  of  SST  and 
TKSLS in R9 and earlier, although in a different way.  Now PENMAX 
corresponds to the maximum penetration depth for solid elements (if 
nonzero, otherwise  it  is  a  characteristic  length).    SLDTHK  is  used  to 
offset  the  contact  surface  from  the  physical  surface  of  the  solid  ele-
ment,  instead  of  playing  with  SST  and  TKSLS,  which  was  rather 
awkward.    This  update  also  saves  the  pain  of  having  to  treat  shells 
and  solids  in  separate  interfaces  if  these  features  are  wanted.    This 
changes the behavior in some inputs that did have SST turned on for 
solids, but a necessary measure to make the contact decent for future 
versions.  
  The  characteristic  length  for  solid  elements  has  been  revised  to  not 
result  in  too  small  sizes  that  would  lead  to  high  contact  stiffnesses 
and less margin for maximum penetration. 
  SFS  on  CONTACT_..._MORTAR  can  be  input  as  negative,  then  con-
tact pressure is the -SFS load curve value vs penetration.  
  Smooth  roundoffs  of  sharp  edges  in  MORTAR  contact  has  been  ex-
tended  to  high  order  segments,  meaning  that  edge  contact  is  valid 
even in this case. 
  The  MORTAR  contact  now  honors  the  NLOC  parameter  for  shells, 
see  *SECTION_SHELL,  adjusting  the  contact  geometry  accordingly.  
Note that CNTCO on *CONTROL_SHELL applies as if always active, 
meaning that if NLOC is on, then CNTCO will also be "on" for MOR-
TAR contacts.
INTRODUCTION 
  Output of contact gaps to the intfor file is now supported for MOR-
TAR contact, see *DATABASE_EXTENT_INTFOR. 
  Transducer  contacts,  *CONTACT_..._FORCE_TRANSDUCER,  are 
supported  for  MORTAR  contact  in  SMP  and  MPP.    A  disclaimer  is 
that  the  slave  and  master  sets  in  the  transducer  have  to  be  defined 
through parts or part sets.  Warnings are issued if this is violated. 
  Option  2 
is  now  supported  for 
tiebreak  MORTAR  contact, 
*CONTACT_..._MORTAR_TIEBREAK,  but  only  for  small  sliding.  
Options  4  and  7  are  supported  in  the  MORTAR  tiebreak  contact  for 
any type of sliding. 
  For explicit analysis, the bucket sort frequency for MORTAR contact 
is  100,  but  can  be  changed  through  parameter  BSORT  on  the  CON-
TACT_..._MORTAR card or NSBCS on CONTROL_CONTACT.  Note 
that the MPP bucket sort parameter does not apply. This assumes to 
improve  the  efficiency  of  MORTAR  explicit  contact  significantly 
compared to R9 and earlier versions. 
  Dynamic  friction  is  supported  in  MORTAR  contact  for  explicit  and 
implicit dynamic analysis.  See FD and DC on *CONTACT_...  card. 
  Wear  calculations  are  supported  for  the  MORTAR  contact.    See 
CONTACT_ADD_WEAR. 
  Triangular shell form 24 is supported with MORTAR forming contact 
and accounts for high order shape functions. 
  Automatic MORTAR contact now supports contact with end faces of 
beam elements and not just the lateral surfaces. 
  Mortar contact is available in 2D plane strain and axisymmetric simu-
lations, but only for SMP implicit.  See CONTACT_2D_...MORTAR. 
◦  Wear computed from *CONTACT_ADD_WEAR can optionally be output 
to  dynain  on  optional  card  of  *INTERFACE_SPRINGBACK_LSDYNA.  
This  will  generate  *INITIAL_CONTACT_WEAR  cards  for  subsequent 
wear simulations, and LS-DYNA will apply this wear and modify geome-
try accordingly.  Restrictions as described in the manual apply. 
◦  Improve 
under 
*CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE  to  allow 
users to define part ID and a node set is automatically generated. 
SOFT = 6 
•  *CONSTRAINED 
◦  Add frictional energy calculation for constraint-based rigid walls. 
◦  *CONSTRAINED_BEAM_IN_SOLID: 
  Works with r-adaptivity now. 
  Can now constrain beams in tshells as well as solids.
INTRODUCTION 
◦  Fix a bug for *CONSTRAINED_LOCAL that might mistakenly constrain z-
translation when RC = 0. 
◦  The  following  options  do  not  support  MEMORY = auto  properly.    The 
MEMORY = auto option will be turned off in this section and report an er-
ror if additional memory allocation is needed. 
*CONSTRAINED_LINEAR_OPTION 
*CONSTRAINED_MULTIPLE_GLOBAL 
◦  Switched translational joints with stiffness to use double precision storage 
for the displacement value so that the calculated forces are more accurate.  
This prevents round-off error that can become significant. 
◦  Fixed  *CONSTRAINED  TIED_NODES_FAILURE  when  used  with  MPP 
single  surface  segment  based  contact.    Non-physical  contact  between  seg-
ments that share tied constraints was being penalized leading to failure of 
the constraints. 
◦  The 
SPR 
(*CONSTRAINED_SPR2, 
*CONSTRAINED_INTERPOLATION_SPOTWELD)  now 
the 
SPOTDEL option of *CONTROL_CONTACT.  That means if shell elements 
involved in the SPR domain fail, the SPR gets deactivated. 
support 
models 
•  *CONTROL 
◦  Fix  possible  error 
◦  Fix  spurious  deletion  of  elements  when  using  TSMIN.ne.0.0 
termination  with  single  precision  MPP  when 
PSFAIL.ne.0 in *CONTROL_SOLID and using solid formulation 10/13/44. 
in 
*CONTROL_TERMINATION,  erode = 1  in  *CONTROL_TIMESTEP  and 
initialized implicitly in dynamic relaxation. 
◦  Added  keyword  *CONTROL_ACOUSTIC  to  calculate  the  nodal  motions 
of *MAT_ACOUSTIC nodes for use in d3plot and time history files.  With-
out this option the *MAT_ACOUSTIC mesh propagates pressure but does 
not  deform  because  it  uses  a  linear  Eulerian  solution  method.    The  struc-
tural response is unaffected by this calculation; it is only for visualization 
and  will  roughly  double  the  time  spent  computing  acoustic  element  re-
sponse. 
◦  When IACC = 1 on *CONTROL_ACCURACY and for shell type 16/-16 in 
nonlinear  implicit,  shell  thickness  change  due  to  membrane  strain  when 
ISTUPD > 0 in *CONTROL_SHELL is now included in the solution process 
and will render continuity in forces between implicit time steps.  The out-
put  contact  forces  will  reflect  the  equilibrated  state  rather  than  the  state 
prior or after the thickness update. 
is  used 
◦  Fix  bug  when  RBSMS  in  *CONTROL_RIGID,  affecting  mass  scaled  solu-
in  conjunction  with  *ELEMENT_INERTIA  and/or 
on 
and 
tions, 
*PART_INERTIA, 
*CONSTRAINED_RIGID_BODIES 
*CONSTRAINED_EXTRA_NODES. 
specifically  with 
choices 
IFLAG 
of 
◦  Tshells added to the subcycling scheme (*CONTROL_SUBCYCLE).
INTRODUCTION 
◦  Tshells  and  spotweld  beams  are  supported  in  selective  mass  scaling.    See 
IMSCL in *CONTROL_TIMESTEP. 
◦  Add  a  new  keyword:  *CONTROL_FORMING_SHELL_TO_TSHELL  to 
convert shell elements to tshell elements. 
  If a parent node has SPCs, the same SPC constraints will be applied to 
the corresponding tshell nodes. 
  If  adaptivity  is  invoked,  *BOUNDARY_SPC_SET  is  automatically 
updated to include newly generated nodes. 
  Allows the normal of the segment set to be changed. 
  Can  offset  the  generated  tshells  from  the  mid-surface  of  the  parent 
shells. 
  Automatically generate segment sets for the top and bottom surfaces, 
which can be used for contact. 
•  DISCRETE ELEMENT METHOD 
◦  Implement 
generalized 
for 
*DEFINE_DE_TO_SURFACE_COUPLING  based  on  the  following  article 
in the journal "Wear": Magnee, A., Generalized law of erosion: application 
to various alloys and intermetallics, Wear, Vol.  181, 500, 1995. 
erosion 
law 
of 
◦  Modify tangential force calculation to get better rigid body rotation behav-
ior for *DEFINE_DE_BOND 
◦  Support  restart  feature  for  DEM  interface  force  file  and  DATABASE  out-
put. 
◦  Instead of using bulk modulus, use mass and time step to estimate contact 
stiffness for SPH-DEM coupling.  This should be better if DEM material is 
quite different from SPH material. 
◦  Fix *DEFINE_DE_MASSFLOW_PLANE bug if DE injection is defined. 
◦  Add CID_RCF to *DEFINE_DE_TO_SURFACE_COUPLING for force out-
put in local coordinates to 'demrcf' file. 
◦  Update the *DEFINE_DE_BY_PART card so that it matches the capabilities 
of the *CONTROL_DISCRETE_ELEMENT card. 
◦  Add  penalty  stiffness  scale  factor,  thickness  scale  factor,  birth  time  and 
death time to *DEFINE_DE_TO_SURFACE_COUPLING. 
◦  Add dynamic coefficient of friction to *CONTROL_DISCRETE_ELEMENT. 
to 
◦  Implement  Finnie's  wear 
law  and  user  defined  wear  model 
*DEFINE_DE_TO_SURFACE_COUPLING. 
◦  Implement user-defined curve for DEM frictional coefficient as function of 
time. 
◦  Implement  user-defined  curve 
for  contact 
force  calculation 
for 
*CONTROL_DISCRETE_ELEMENT. 
◦  Fix 
inconsistent 
results 
between 
*DEFINE_DE_BY_PART 
and 
*CONTROL_DISCRETE_ELEMENT.
INTRODUCTION 
•  *ELEMENT 
◦  Fixed bug affecting output from beam elements ELFORM = 2 when certain 
uncommon  inputs  are  present.    Forces  and  moments  in  the  output  files 
could  be  wrongly  rotated  about  the  beam  axis.    This  affected  the  output 
files only, not the solution inside LS-DYNA.  The error could occur under 
two circumstances: (a) if IST on *SECTION_BEAM is non-zero, the output 
forces  and  moments  are  supposed  to  be  rotated  into  the  beam's  principal 
axis  system,  but  this  rotation  could  be  applied  to  the  wrong  beam  ele-
ments; and (b) when no ELFORM = 2 elements have IST, but the model al-
the 
so  contains  beams  with  ELFORM = 6  and  RRCON = 1  on 
SECTION_BEAM  card,  some  of  the  ELFORM = 2  elements  can  have  their 
output forces and moments rotated by 1 radian. 
◦  Fix a bug affecting 2d seatbelt with time-dependent slipring friction. 
◦  Fix erroneous 1d seatbelt slipring message. 
◦  Fix seatbelt consistency issue in SMP (ncpu < 0). 
◦  Add error message when 2d seatbelt part doesn't have shell formulation of 
5 and *MAT_SEATBELT. 
◦  Fix a bug for 2d seatbelt that could occur when a model has both 1d and 2d 
belts, and a 1d pretensioner of type 2, 3 or 9. 
◦  Fix an MPP seatbelt bug that could occur when using a type 9 pretension-
er. 
◦  Allows shell formulation 9 to be used for 2d seatbelt.  It was reset to formu-
lation 5 by LS-DYNA, no matter what formulation was input.  Now, only 
formulation  5  and  9  are  accepted  as  input.   Other  formulations  will  incur 
error message. 
◦  MPP now supports *ELEMENT_MASS_MATRIX_NODE_(SET). 
◦  Added  cohesive  shell  formulation  -29.    This  formulation  uses  a  cohesive 
midlayer  where  local  direction  q1  coincides  with  the  average  of  the  sur-
rounding  shell  normals.    This  formulation  is  better  suited  for  simulating 
normal shear. 
◦  Cohesive shell formulation +/-29: Fixed absence of part mass in d3hsp. 
◦  Make *TERMINATION_DELETED_SOLIDS work with hex spot weld fail-
ures. 
◦  Fix  incorrect  load  curve  used  if  large  value  is  used  for  FC < 0  and/or 
FCS < 0 in *ELEMENT_SEATBELT_SLIPRING. 
◦  Fix incorrect velocity on accelerometer if  
  velocity  is  prescribed  on  the  rigid  body  that  the  accelerometer  is  at-
tached to, and 
  INTOPT = 1 in *ELEMENT_SEATBELT_ACCELEROMETER, and 
  *INITIAL_VELOCITY_GENERATION_START_TIME is used. 
◦  Fix incorrect discrete spring behavior when used with adaptivity.
INTRODUCTION 
◦  Fix input error when using *DEFINE_ELEMENT_DEATH with BOXID > 0 
for MPP. 
◦  Modify  tolerances  on  error  messages  SOL+865  and  SOL+866  to  prevent 
unnecessary  error  terminations  when  translational  or rotational  mass  of  a 
discrete beam was close to zero. 
◦  Made the solid element negative volume warning SOL+630 for penta for-
mulatgion 15 consistent with the volume calculation in the element.  With 
this change, elements are deleted rather than the job terminating with error 
SOL+509. 
◦  Fixed the default hourglass control for shell form 16.  It was defaulting to 
type 5 hourglass control rather than 8. 
◦  Fixed  default  hourglass  control  when  the  *HOURGLASS  control  card  is 
used but no HG type is specified.  We were setting to type 1 instead of 2.  
Also,  fixed  the  default  HG  types  to  match  the  user's  manual  for  implicit 
and explicit. 
◦  Fixed  the  fully  integrated  membrane  element  (shell  ELFORM = 9)  when 
used with NFAIL4 = 1 on *CONTROL_SHELL and there are triangular el-
ements  in  the  mesh.    Triangular  elements  were  being  deleted  by  the  dis-
torted element check. 
◦  Fixed  a  divide  by  zero  error  that  occurred  with  *SECTION_BEAM, 
-12,  and  node  3  was  omitted  on 
ELFORM = 6,  SCOOR = 12  or 
*ELEMENT_BEAM, and nodes 1 and 2 are along the global y-direction or 
z-direction. 
◦  Fixed  laminated  shell  theory  for  type  6  and  7  shell  elements  when  made 
active by LAMSHT = 3 or 5 on *CONTROL_SHELL. 
◦  Added  an 
int.pt. 
  variable 
for  *PART_COMPOSITE_LONG  and 
*PART_COMPOSITE_TSHELL_LONG  called  SHRFAC  which  is  a  scale 
factor  for  the  out-of-plane  shear  stress  that  allows  the  user  to  choose  the 
stress distribution through thickness.  This was motivated by test data that 
shows  that  for  large  differences  is  layer  shear  stiffness,  the  parabolic  as-
sumption is poor. 
◦  Fixed implicit hourglass stiffness in viscoelastic materials when used with 
tshell forms 5 or 6.  The stiffness was much too small. 
◦  Modified tshell type 5 to use the tangent stiffness for calculating the Pois-
son's affects and hourglass control for *MAT_024.  This makes the behavior 
softer during buckling which is much more realistic. 
◦  Fixed  a  significant  bug  in  segment  based  contact  when  SHLEDG = 1  and 
SBOPT = 3  or  5  and  DEPTH < 45,  and  shell  segments  in  contact  have  dif-
ferent  thicknesses.    A  penetration  check  was  using  incorrect  thicknesses 
causing contact to be detected too late, particularly for edge to surface con-
tact. 
◦  Improved the time step calculation for triangular tshell elements.  The time 
step was too conservative for elements with significant thickness.  This fix 
does not affect tshell type 7.
INTRODUCTION 
◦  Fixed all tshells to work with anisotropic thermal strains which can be de-
fined by *MAT_ADD_THERMAL.  Also, this now works by layer for lay-
ered composites. 
◦  Enabled tshell form 5 to recalculate shear stiffness scale factors when plas-
ticity material models 3, 18, 24, 123, or 165 are included in a composite sec-
tion.  Prior to this change the scale factors were based on elastic properties 
so after yielding, the stress distribution was not what was expected.  This 
new  capability  supports  the  constant  stress  option,  the  parabolic  option, 
and the SHRFAC option on *PART_COMPOSITE_TSHELL_LONG. 
◦  Improved tshell 5 when used with mixed materials in the layers.  A failure 
to use the correct Poisson's ratio was causing a less accurate stress tensor. 
◦  Modified the time step calculation for tshell forms 3 and 5.  A dependence 
on  volumetric  strain  rate  was  removed  in  order  to  prevent  oscillations  in 
the time step which caused stability problems, particularly for tshell 5. 
(TSHEAR = 1 
on 
*SECTION_TSELL or *PART_COMPOSITE).  It was producing a not very 
constant stress distribution. 
constant 
◦  Fixed 
option 
stress 
tshell 
shear 
◦  Fixed stress and strain output of tshells when the composite material flag 
CMPFLG  is  set  on  *DATABASE_EXTENT_BINARY.    The  transformation 
was backwards. 
mass 
when 
*ELEMENT_SHELL_SOURCE_SINK  is  used.    The  mass  of  inactive  ele-
ments was being included. 
reported 
◦  Fixed 
d3hsp 
parts 
of 
to 
◦  Enabled *MAT_026 and *MAT_126 (HONEYCOMB) to be used with tshell 
forms 3, 5, and 7.  It was initialized incorrectly causing a zero stress. 
◦  Added a missing internal energy calculation for tshell form 6. 
◦  Enabled tshell forms 1, 2, and 6 to work with material types 54, 55, and 56. 
◦  Modified  the  z-strain  distribution  in  tshell  forms  5  and  6  when  used  in 
composites with mixed materials that are isotropic.  The existing assumed 
strain scheme was doing a poor job of creating a constant z-stress through 
the thickness. 
◦  Increased the explicit solution time step for thin shell composite elements.  
The existing method calculated a sound speed using the stiffness from the 
stiffest layer and dividing it by the average density of all layers.  This could 
be overly conservative for composites with soft layers of low density.  The 
new method uses the average stiffness divided by average density.  This is 
still conservative, but less so. 
◦  Corrected rotational inertia of thin shells when layers have mixed density 
and the outer layers are denser than inner layers.  The fix will mostly affect 
elements that are very thick relative to edge length. 
◦  Added  support  for  *ELEMENT_SHELL_SOURCE_SINK  to  type  2  shells 
with BWC = 1 on *CONTROL_SHELL. 
◦  Prevent 
(from 
shell 
*ELEMENT_SHELL_SOURCE_SINK)  from  controlling  the  solution  time 
step. 
elements 
inactive
INTRODUCTION 
◦  Fixed  *LOAD_STEADY_STATE_ROLLING  when  used  with  shell  form  2 
(BWC = 1 
Belytschko-  Wong-Chang  warping 
and 
*CONTROL_SHELL).  The load was not being applied. 
stiffness 
◦  Improved the brick element volume calculation that is used by the option 
erode elements (ERODE = 1 on *CONTROL_TIMESTEP or PSFAIL.ne.0 on 
*CONTROL_SOLID).    It  was  not  consistent  with  the  element  calculation 
which caused an error termination. 
◦  Fixed  all  tshell  forms  to  work  with  anisotropic  thermal  strains  which  can 
be defined by *MAT_ADD_THERMAL.  Also, this now works by layer for 
layered composites. 
◦  Reworked shell output so that we can correctly output stress in triangular 
shells  when  triangle  sorting  is  active,  that  is  when  ESORT = 1  or  2  on 
*CONTROL_SHELL. 
◦  *ELEMENT_T/SHELL_COMPOSITE(_LONG) 
and 
*PART_COMPOSITE_T/SHELL_(LONG):  Permit  the  definition  of  zero 
thickness layers in the stacking sequence.  This allows the number of inte-
gration points to remain constant even as the number of physical plies var-
integration  point 
ies  and  eases  post-processing  since  a  particular 
corresponds  to  a  physical  ply.    Such  a  capability  is  important  when  plies 
are not continuous across a composite structure. 
To  represent  a  missing  ply,  set  THK  to  0.0  for  the  corresponding  integra-
tion  point  and  additionally,  either  set  MID = -1  or  set  PLYID  to  any  non-
zero  value.    Obviously,  the  PLYID  option  applies  only  to  the  keywords 
containing LONG. 
◦  Implemented  sum  factorization  for  27-node  quadratic  solid  that  may  in-
crease speed by a factor of 2 or 3. 
◦  Support  second  order  solid  elements  (formulations  23,24,25,26)  for 
*SET_NODE_GENERAL. 
◦  Invoke consistent mass matrix of 27-node hex element for implicit dynam-
ics and eigenvalues. 
◦  Reorder  node  numbering  when  assembling  global  stiffness  matrix  for  27-
node hex.  This fixes a bug in which it  was reported than the implicit 27-
node element didn't work 
◦  Automatically  transfer  nodal  boundary  conditions  for  newly  generated 
nodes if H8TOH27 option is used in *ELEMENT_SOLID. 
◦  Modify initialization of material directions for solid elements.  If there are 
only zeros for all the 6 values in *INITIAL_STRESS_SOLID, then the values 
from the other input (e.g.  *ELEMENT_SOLID_ORTHO) are kept. 
◦  Enable *PART_STACKED_ELEMENTS to pile up shell element layers.  Be-
fore, it was necessary that solid element layers were placed between shell 
element  layers.    Now,  shell  element  layers  can  follow  each  other  directly.  
Contact definitions have to be done separately. 
◦  Allow  *PART_STACKED_ELEMENTS  to  be  used  in  adaptive  refinement 
simulations.
INTRODUCTION 
◦  Add alternative mass calculation for critical time step estimate of cohesive 
elements.  This hopefully resolves rarely occurring instability issues.  Op-
tion ICOH on *CONTROL_SOLID is used for that. 
◦  Correct the strain calculation for tet formulation 13.  This did not affect the 
stress response, only output of strains.  Nodal averaging was not account-
ed for. 
◦  User 
defined 
*SECTION_SHELL/SOLID) 
*MAT_ADD_EROSION. 
elements 
(ELFORM = 101 
can 
now 
be  used 
to 
105 
on 
together  with 
◦  Add  option 
to  define  a  pull-out 
in 
*ELEMENT_BEAM_SOURCE  by  defining  a  negative  variable  FPULL.  
|FPULL| 
or 
refer 
*DEFINE_CURVE_FUNCTION. 
*DEFINE_CURVE 
time  curve 
force  vs. 
can 
to 
◦  Solid  tet  form  13  supported  for  all  materials  in  implicit,  including  a  pre-
sumable consistency improvement for the future. 
◦  The Hughes-Liu beam is supported in *INTEGRATION_BEAM such each 
integration point may refer to a different part ID and thus have a different 
coef.  Of thermal expansion.  See *MAT_ADD_THERMAL_EXPANSION. 
◦  Shell  types  2  and  16  that  combines  thermal  expansion  and  thick  thermal 
shells,  see  *MAT_ADD_THERMAL_EXPANSION  and  TSHELL  on 
*CONTROL_SHELL, now correctly treat temperature gradient through the 
thickness to create bending moments.  All shell types are to be supported 
in due time. 
◦  *SECTION_BEAM_AISC  now  provides  predefined  length  conversion  fac-
tors for specific unit systems. 
◦  3D tet r-adaptivity now supports *DEFINE_BOX_ADAPTIVE. 
  For  every  adaptive  part,  users  can  define  multiple  boxes  where  dif-
ferent  BRMIN  &  BRMAX  (corresponding  to  RMIN  &  RMAX  in 
*CONTROL_REMESHING)  can  be  specified  for  3D  tet  remesher  to 
adjust the mesh size. 
  Current implementation does not support LOCAL option. 
◦  Fix  bug  in  3D  adaptivity  so  that  users  can  now  have  both  non-adaptive 
tshell parts and 3D adaptive parts in one analysis. 
◦  Fix  the  bug  in  3D  adaptivity  so  that  users  can  now  have  both  dummy 
nodes and 3D adaptive parts in one analysis. 
•  *EM (Electromagnetic Solver) 
◦  Randles Circuits for Battery Modeling 
  A Randles circuit is an equivalent electrical circuit that consists of an 
active electrolyte resistance r0 in series with the parallel combination 
of the capacitance c10 and an impedance r10.  The idea of the distrib-
INTRODUCTION 
uted Randles model is to use a certain number of Randles circuits be-
tween corresponding nodes on the two current collectors of a battery 
unit  cell.    These  Randles  circuits  model  the  electrochemistry  that 
happens  in  the  electrodes  and  separator  between  the  current  collec-
tors.    The  EM  solver  can  then  solve  for  the  EM  fields  in  the  current 
collectors, and the connections between them. 
  Added analysis of distributed Randles circuits to MPP. 
  Added d3plot output for distributed Randles circuits: 
  D3PL_RAND_r0_EM, 
  D3PL_RAND_r10_EM, 
  D3PL_RAND_c10_EM, 
  D3PL_RAND_soc_EM, 
  D3PL_RAND_i_EM, 
  D3PL_RAND_u_EM, 
  D3PL_RAND_v_EM, 
  D3PL_RAND_vc_EM, 
  D3PL_RAND_temperature_EM, 
  D3PL_RAND_P_JHR_EM, 
  D3PL_RAND_P_dudt_EM, 
  D3PL_RAND_i_vector_EM 
This  output  can  be  visualized  in  LS-PrePost  versions  4.3  and  4.5  on 
the 
using 
Post/FriComp/Extend/EM node. 
separator 
battery 
part 
cell 
the 
of 
  Added tshells for EM analysis for use in battery modeling. 
  Added  new  capability  for  modeling  Randles  short,  based  on 
*DEFINE_FUNCTION so that the user has a lot of freedom to define 
where and when the short happens as well as the short resistance. 
  Added  a  new  capability  for  battery  exothermal  reactions  also  based 
on 
keyword 
*RANDLE_EXOTHERMAL_REACTION  makes  it  possible  to  com-
plement  the  heating  of  a  short  circuit  created  by  a  short  by  exother-
mal reactions if, for example, the temperature becomes higher than a 
threshold value. 
*DEFINE_FUNCTION. 
new 
The 
•  FORMING ANALYSIS 
◦  Extend  *INCLUDE_AUTO_OFFSET  to  solid  and  beam  elements  (draw 
beads). 
◦  Add 
a 
for 
new 
keyword 
compensa-
tion:*INTERFACE_COMPENSATION_NEW_REFINE_RIGID to refine and 
break rigid tool mesh along the user supplied trim curves so compensated 
tool  mesh  follows  exactly  the  blank  mesh  (file  "disp.tmp").    This  needs  to 
be  done  only  once  in  the  beginning  of  the  springback  compensation  (IT-
ER0). 
springback 
◦  *CONTROL_FORMING_ONESTEP:
INTRODUCTION 
  Change  the  default  element  formulation  option  for  onestep  method 
to QUAD2. 
  Add a new option QUAD to allow quadrilateral elements to be con-
sidered. 
  Limit  the  maximum  thickening  by  using  a  new  variable  TSCLMAX 
for the sheet blank. 
  Set  the  value  of  OPTION  to  a  negative  value  to  output  the  file  'on-
estepresult' in large format (E20.0). 
  Calculate  and  add  the  damage  factor  and  output  to  the  6th  history 
variable  in  the  output  file  "onestepresult".    Add  the  variable  for  a 
curve ID to define the fracture strain vs.  triaxility.  Add another vari-
able DMGEXP (damage parameter), as used in GISSMO model. 
  Keep the original coordinates for the onestep output "onestepresults". 
◦  Add a new option VECTOR to *CONTROL_FORMING_BESTFIT to output 
deviation vector (in the format of: NODEID, xdelta, ydelta, zdelta) for each 
node to its closest target element.  The deviation vectors are output under 
the keyword *NODE_TO_TARGET_VECTOR. 
◦  *CONTROL_FORMING_OUTPUT: 
  Output will skip any negative abscissa (Y1) value. 
  When  CIDT < 0,  the  positive  value  defines  the  time  dependent  load 
curve. 
◦  Add 
a 
warning 
compensation 
*INTERFACE_SPRINGBACK_COMPENSATION  to  identify  which  input 
file  (typically  the  blank  with  adaptive  mesh  not  output  directly  by  LS-
DYNA) has the wrong adaptive constraints. 
springback 
in 
◦  *INTERFACE_COMPENSATION_3D: turn off the output of nikin file. 
◦  *ELEMENT_LANCING: 
  Allow some unused lancing curves to be included in the input. 
  When  the  gap  between  the  two  ends  of  a  lancing  curve  is  not  zero, 
but small enough, then this curve is automatically closed. 
  Allow  several  parts  to  be  cut  during  lancing;  the  parts  can  be 
grouped  in  *SET_PART_LIST,  and  defined  using  a  negative  value 
IDPT. 
  Specify  the  distance  to  bottom  dead  center  as  AT  and  ENDT  when 
the new variable CIVD is defined. 
  Set  IREFINE = 1  (default)  in  lancing,  to  refine  blank  mesh  automati-
cally along the lancing curves. 
  Re-set the adaptive level to be 1 to prevent those elements along the 
lancing route to be further refined.
INTRODUCTION 
  When IREFINE = 1, elements along the lancing curve will be refined 
to make sure that no adapted nodes exist in the neighborhood.  This 
helps get improved lancing boundary. 
  Change of tolerance for lancing to merge the small elements into big-
ger ones. 
◦  Add a new keyword to perform trimming after lancing (shell elements on-
ly): *DEFINE_LANCE_SEED_POINT_COORDINATES.  Maximum of two 
seed nodes can be defined. 
◦  Extend  *CONTROL_FORMING_TOLERANC  to  *MAT_036,  *MAT_037, 
*MAT_125, and *MAT_226. When beta is less than -0.5, there is no necking 
and  no  calculation  of  FI.  When  beta  is  greater  than  1.0,  beta = 1.0/beta. 
This keyword adds a smoothing method to calculate the strain ratios for a 
better formability index. 
◦  Sandwiched parts (*CONTROL_ADAPTIVE, *DEFINE_CURVE_TRIM): 
  Disable  *CONTROL_ADAPTIVE_CURVEs  for  sandwich  parts,  since 
refinement along the curve is automatically done during trimming. 
  Refine the elements along the trimming curve to make sure no slave 
nodes are be cut by trimming curves. 
  Allow mesh adaptivity. 
  Allow multi-layers of solids. 
  Add a check to the variable IFSAND in *CONTROL_ADAPTIVE for 
sandwich part to be refined to exclude solid elements. 
◦  Solid element trimming (*DEFINE_CURVE_TRIM): 
  Refine those elements along the trimming curve. 
  Improve  solid  trimmig  to  allow  the  trimming  of  one  panel  into  two 
panels with two seed nodes. 
◦  Add 
a 
keyword 
*CONTROL_FORMING_REMOVE_ADAPTIVE_CONSTRAINTS 
re-
move adaptive constraints on a formed, adapted blank, and replaced them 
with triangular elements. 
new 
to 
◦  *DEFINE_CURVE_TRIM_NEW: Allow trimming of tshells. 
◦  Add  a  new  keyword:*INTERFACE_WELDLINE_DEVELOPMENT  to  ob-
tain initial weld line from the final part and the final weld line position. 
  When Ioption = -1, convert weld line from its initial position to the fi-
nal part. 
  Output the element nodes that intersect the weld line in the final part, 
and the output file is: affectednd_f.ibo 
  Output  the  element  nodes  that  intersect  the  weld  line  in  the  initial 
part, and the output file is: affectednd_i.ibo
INTRODUCTION 
◦  Add a new variable DT0 to *CONTROL_IMPLICIT_FORMING so there is 
no need to use *CONTROL_IMPLICIT_GENERAL to specify DT0. 
◦  *INTERFACE_BLANKSIZE: 
  Add  a  new  feature  DEVELOPMENT  option.    When  ORIENT = 2, 
then  a  reference  mesh  file  for  the  formed  part  should  be  included.  
The  calculated  and  compensated  boundary will  be  based  on  the  ref-
erence mesh. 
  Add a new option SCALE_FACTOR that allows the target curve to be 
moved.  This  is  useful  when  multiple  target  curves  (e.g.    holes)  and 
formed curves are far away from each other. 
•  *FREQUENCY_DOMAIN  
◦  Added  new  keyword  *CONTROL_FREQUENCY_DOMAIN  to  define 
global  control  parameters  for  frequency  domain  analysis.    Currently  two 
parameters are defined: 
  REFGEO: flag for reference geometry in acoustic eigenvalue analysis 
(either the original geometry at t = 0, or the deformed geometry at the 
end of transient analysis). 
  MPN:  large  mass  added  per  node,  to  be  used  in  large  mass  method 
for enforced motion. 
◦  *FREQUENCY_DOMAIN_ACOUSTIC_BEM: 
  Enabled 
wave 
(*FREQUENCY_DOMAIN_ACOUSTIC_INCIDENT_WAVE)  in  Ray-
leigh method (METHOD = 0). 
incident 
using 
  Enabled 
plot 
(*FREQUENCY_DOMAIN_ACOUSTIC_FRINGE_PLOT)  in  Rayleigh 
method (METHOD = 0). 
pressure 
acoustic 
fringe 
  Fixed bug in running  acoustic analysis with  multiple boundary con-
ditions in MPP. 
  Fixed running MATV (Modal Acoustic Transfer Vector) approach in 
MPP (*FREQUENCY_DOMAIN_ACOUSTIC_BEM_MATV). 
  Added  treatment  for  triangular  elements  used  in  Rayleigh  method 
(METHOD = 0). 
  Added  output  of  acoustic  intensity  to  binary  database  D3ACS  (de-
fined by *DATABASE_FREQUENCY_BINARY_D3ACS). 
  Fixed  bug  in  acoustic  pressure  fringe  plot  for  collocation  BEM 
(METHOD = 3)  and  dual  BEM  based  on  Burton-Miller  formulation 
(METHOD = 4). 
◦  *FREQUENCY_DOMAIN_ACOUSTIC_FEM:
INTRODUCTION 
  Fixed bug in acoustic analysis by FEM, when dimensions of mass and 
k (stiffness) matrices are mismatched. 
◦  *FREQUENCY_DOMAIN_ACOUSTIC_FRINGE_PLOT: 
  Implemented  acoustic  fringe  plot  for  MPP  for  the  options  PART, 
PART_SET, and NODE_SET. 
◦  *FREQUENCY_DOMAIN_FRF: 
  Added new loading types: 
VAD1 = 5: enforced velocity by large mass method 
            = 6: enforced acceleration by large mass method 
            = 7: enforced displacement by large mass method 
            = 8: torque 
            = 9: base angular velocity 
           = 10: base angular acceleration 
           = 11: base angular displacement 
  Added rotational dof output for FRF. 
◦  *FREQUENCY_DOMAIN_MODE: 
  Added option _EXCLUDE to exclude some eigenmodes in modal su-
perposition in frequency domain analysis. 
◦  *FREQUENCY_DOMAIN_RANDOM_VIBRATION: 
  Fixed bug in running random vibration with random pressure wave 
load (VAFLAG = 2) in MPP. 
  Improved random vibration analysis by allowing using complex var-
iable cross PSD functions.  Previously cross PSD was defined as real 
variables thus the phase difference was ignored. 
  Added PSD and RMS computation for Von Mises stress in beam ele-
ments. 
◦  *FREQUENCY_DOMAIN_RESPONSE_SPECTRUM: 
  Added  Von  Mises  stress  output  for  beam  elements  in  database 
D3SPCM. 
  Corrected  computation  of  response  spectrum  at  an  intermediate 
damping  value  by  interpolating  spectra  at  two  adjacent  damping 
values.  Now the algorithm is based on ASCE 4-98 standard. 
◦  *FREQUENCY_DOMAIN_SSD: 
  Added new loading types: 
VAD = 5: enforced velocity by large mass method
INTRODUCTION 
          = 6: enforced acceleration by large mass method 
          = 7: enforced displacement by large mass method 
          = 8: torque 
  Fix 
for 
running  SSD 
fatigue 
in  MPP 
(affected  keyword: 
*FREQUENCY_DOMAIN_SSD_FATIGUE). 
  Updated  ssd  computation  with  local  damping,  and  enabled  the  re-
start feature by reading damping matrix. 
  Implemented  ERP 
(Equivalent  Radiated  Power, 
keyword 
*FREQUENCY_DOMAIN_SSD_ERP) for MPP. 
◦  *DATABASE_FREQUENCY_ASCII: 
  Added  keyword  *DATABASE_FREQUENCY_ASCII_{OPTION}  to 
define  the  frequency  range  for  writing  frequency  domain  ASCII  da-
and 
tabases  NODOUT_SSD, 
ELOUT_PSD. 
ELOUT_SSD,  NODOUT_PSD 
•  *ICFD (Incompressible Fluid Solver) 
◦  New ICFD features and major modifications 
  Simple restart is now supported for ICFD. 
  Added 
damping 
wave 
capabilities. 
See 
*ICFD_DEFINE_WAVE_DAMPING. 
  Added  steady  state  solver.    See  *ICFD_CONTROL_GENERAL  and 
*ICFD_CONTROL_STEADY. 
steady 
  Added 
state 
potential 
flow 
solver. 
See 
*ICFD_CONTROL_GENERAL. 
  Weak thermal coupling for conjugate heat transfer is now possible in 
See 
classic  monolithic 
approach. 
addition 
to 
*ICFD_CONTROL_CONJ. 
the 
  Windkessel  boundary  conditions  are  now  available  for  blood  flow.  
See *ICFD_BOUNDARY_WINDKESSEL. 
  It  is  now  possible  to  output  the  heat  transfer  coefficient  as  a  surface 
variable in LSPP or in ASCII format on segment sets for a subsequent 
solid-thermal only analysis.  See *ICFD_DATABASE_HTC. 
  Two  way  coupling  is  now  possible  with  DEM  particles.    See 
*ICFD_CONTROL_DEM_COUPLING. 
  Modifications  introduced  in  the  SUPG  stabilization  term  used  in 
thermal and conjugate heat transfer problems for improved accuracy 
and speed. 
◦  Additions and modifications to existing ICFD keywords 
  *ICFD_BOUNDARY_FSWAVE:
INTRODUCTION 
Added a boundary condition for wave generation of 2nd order stokes 
waves with free surfaces 
  *ICFD_CONTROL_FSI:  
Added  a  flag  which,  when  turned  on  will  project  the  nodes  of  the 
CFD  domain  that  are  at  the  FSI  interface  onto  the  structural  mesh.  
This is recommended for cases with rotation. 
  *ICFD_CONTROL_MESH:  
Added a flag to allow the user control over whether there will be re-
mesh  or  not.    If  there  is  no  re-mesh  then  we  can  free  space  used  to 
backup the mesh and lower memory consumption. 
  *ICFD_CONTROL_MESH_MOVE: 
Added option to force the solver to turn off any mesh displacements.  
This can be useful in cases where the mesh is static to save a little bit 
of calculation time. 
  *ICFD_CONTROL_OUTPUT: 
Added  option  to  support  output  in  Fieldview  format,  binary  and 
ASCII. 
When output of the fluid volume mesh is requested, the mesh will be 
divided into ten distinct parts, grouping elements in ten deciles based 
on the mesh quality (Part 1 has the best quality elements, part 10 the 
worst). 
  *ICFD_CONTROL_POROUS: 
Improvements for RTM problems. 
  *ICFD_CONTROL_TIME: 
Added an option to define an initial timestep. 
Added  an  option  to  shut  off  the  calculation  of  Navier  Stokes  after  a 
certain  time  leaving  only  the  heat  equation.    This  can  be  useful  to 
save calculation times in conjugate heat transfer cases where the fluid 
often reaches steady state before the thermal problem. 
  *ICFD_DATABASE_DRAG: 
It is now possible to output the force on segment sets in a FSI run di-
rectly in LS-DYNA compatible format.  This can be useful for a sub-
sequent linear FSI analysis running only the solid mechanics part. 
Added flag to output drag as a surface variable in LSPP. 
  *ICFD_DATABASE_FLUX: 
Added option to change output frequency 
  *ICFD_DATABASE_NODOUT: 
The user node IDs are now required rather than the internal node IDs 
  *ICFD_CONTROL_IMPOSED_MOVE: 
Added the option to choose between imposing the displacements  or 
the velocity. 
  *ICFD_CONTROL_TRANSIENT: 
Choose implicit time integration scheme for NS. 
  *ICFD_CONTROL_DEM_COUPLING:
INTRODUCTION 
Added a scale factor for the sphere radius in the computation of the 
DEM force. 
  *ICFD_MODEL_POROUS: 
Added a scale factor option on the permeability for model 1 and 2.  A 
*DEFINE_FUNCTION can also be used. 
  *MESH_BL: 
Added  option  to generate  boundary  layer  mesh  using  a  growth  fac-
tor. 
◦  ICFD bug fixes and minor improvements 
  Fixed  bug  when  multiple  *DEFINE_FUNCTIONs  were  used  in  an 
ICFD problem.  Only the last one was taken into account. 
  LES turbulence model: fixed van Driest damping issue in the bound-
ary layer.  LES models can use wall functions. 
  RANS  turbulence  models:  Standard  k-epsilon,  realizable  k-epsilon, 
Wilcox k-omega uses HRN laws of the wall by default while SST and 
Spalart Allmaras use LRN.  Improvements on the convergence of all 
those models. 
  The  DEM  particle  volume  is  now  taken  into  account  in  free  surface 
problems. 
  Average shear is now output as a surface variable in the d3plots. 
  *ICFD_CONTROL_MONOLITHIC 
(replaced 
*ICFD_CONTROL_GENERAL). 
obsolete 
is 
by 
  Added  more  output  for  the  mesh  generation  indicating  the  stage  of 
the meshing process and the amount of elements that are being gen-
erated as a multiple of 10000.  Added progress % for the extrusion of 
the mesh during the BL mesh generation. 
  Improvements on the element assemble speed in MPP. 
  Fixed  synchronization  problem  for  the  last  timestep  in  an  FSI  prob-
lem. 
  More options have been added to the timer output. 
  Correction of the calculation of the flux in *ICFD_DATABASE_FLUX 
in free surface cases. 
  Boundary layer mesh can go through free-surfaces or mesh size inter-
faces. 
  The  Center  of  Gravity  of  the  fluid  is  output  in  the  icfd_lsvol.dat 
ASCII file in free surface problems 
•  Implicit (Mechanical) Solver 
◦  Enhanced  termination  of  MPP  eigensolver  when  non  eigenmodes  are 
found.
INTRODUCTION 
◦  Implicit was enforcing birth and death times on *BOUNDARY_SPC during 
dynamic  relaxation  contrary  to  the  User's  Manual.    These  times  are  now 
ignored by implicit during dynamic relaxation. 
◦  Corrected  output  of  eigenvalues  and  frequencies  to  file  eigout  for  the 
asymmetric eigenvalue problem. 
◦  Enhanced  logic  that  determines  when to  write  out  the  last  state  to  d3plot 
for implicit. 
◦  Improved error message for reading d3eigv file for *PART_MODES for the 
case when the user inputs a d3eigv file from a different model than intend-
ed. 
◦  Corrected the reporting of kinetic and internal energy in file glstat for im-
plicit. 
◦  Applied  corrections  to  tied  contact  in  implicit  (MPP).    This  affects  slave 
nodes coming from other processes. 
◦  Corrected  output  to  file  d3iter  (implicit  nonlinear  search  vectors)  for  re-
start. 
◦  Enhanced termination process when the implicit solver determined an ear-
ly termination. 
◦  When implicit springback was following an explicit transient step, the im-
plicit  keywords  with  the  _SPR  were  not  properly  handled.    This  is  now 
corrected. 
◦  Added 
a 
warning 
of 
*CONSTRAINED_RIGID_BODY_STOPPERS  and  the  Lagrange  multiplier 
formulation for joints (*CONTROL_RIGID) for explicit.  The warning rec-
ommends switching to the penalty joint formulation. 
combined 
about 
use 
the 
◦  Applied  numerous  bug  fixes  to  the  implicit  solver  associated  with 
*CONSTRAINED_INTERPOLATION where there are lots of independent 
degrees-of-freedom. 
◦  Corrected initialization of MPP tied contact with implicit mechanics when 
the implicit phase follows explicit dynamic relaxation. 
◦  Fixed  an  implicit  problem  where  a  linear  implicit  analysis  follows  inertia 
relief computation. 
◦  Added  gathering  of  damping  terms  from  discrete  elements  from  implicit 
especially for FRF computations and matrix dumping. 
◦  Fixed  Implicit  for  the  case  of  multi-step  Linear  (NSOLVR = 1)  with  Inter-
mittent Eigenvalue Computation. 
◦  Corrected the output to d3iter when 10-noded tets are present. 
◦  Keypoints specified in *CONTROL_IMPLICIT_AUTO are now enforced at 
the initial time step and on restart from explicit. 
◦  Skip  frequency  damping  during  implicit  static  dynamic  relaxation,  i.e.  
IDRFLAG > 5. 
◦  *CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS: 
  The  VID  of  the  rotating  axis  can  now  be  defined  by  both 
*DEFINE_VECTOR  and  *DEFINE_VECTOR_NODES.    It  enables  the
INTRODUCTION 
movement of the rotating axis.  Previously, only *DEFINE_VECTOR 
could be used to define the VID. 
  The rotational dynamics now work in MPP. 
◦  Shell  forms  23  and  24  (high  order  shells),  1D  seatbelts,  Hughes-Liu  and 
spotweld beams (types 1 and 9) are now supported with the implicit accu-
racy  option  (IACC = 1  in  *CONTROL_ACCURACY)  to  render  strong  ob-
jectivity  for  large  rigid  body  rotations.    Also,  shell  type  16  is  supported 
with  implicit  accuracy  option,  resulting  in  forms  16  and  -16  giving  the 
same solution. 
◦  Translational and generalized stiffness joints are now strongly objective for 
implicit analysis.  See CONSTRAINED_JOINT_STIFFNESS.... 
◦  In  implicit  it  may  happen  that  the  initial  loads  are  zero,  for  instance  in 
forming problems.  In addition, the goal is to move a tool in contact with a 
workpiece,  and  the  way  line  search  and  convergence  works,  it  is  hard  to 
get things going.  We now attempt to handle this situation by automatical-
ly  associating  an  augmented  load  to  the  prescribed  motion  simply  to  get 
off the ground. 
◦  New  tolerances  on  maximum  norms  are  introduced  for  convergence  in 
implicit:  ratio  of  max  displacement/energy/residual,  and  absolute  values 
of  nodal  and  rigid  body  translation/rotational  residual  can  be  specified. 
See  DNORM.LT.0  on  *CONTROL_IMPLICIT_SOLUTION  for  defining  an 
additional card for these parameters DMTOL, EMTOL and RMTOL.  Fur-
thermore, maximum absolute tolerances on individual nodal or rigid body 
parameters  can  be  set  on  NTTOL,  NRTOL,  RTTOL  and  RRTOL  on  the 
same card. 
◦  If ALPHA < 0 on first *CONTROL_IMPLICIT_DYNAMICS card, the HHT 
implicit time integration scheme is activated. 
•  *INITIAL 
◦  Fix 
*INITIAL_VELOCITY_GENERATION 
with 
*INCLUDE_TRANSFORM,  which  was  broken  due  to  misplaced  condi-
tionals in r100504. 
when 
used 
◦  Fix  3  bugs  for  *INITIAL_VELOCITY_GENERATION  involving  omega > 0 
and icid > 0: 
  When nx = -999.  Now the directional cosine defined by node NY  to 
node  NZ  will  be  the  final  direction  to  rotate about.    In  other  words, 
the  direction  from  node  NY  to  node  NZ  will  not  be  projected  along 
icid any more. 
  When  nx  !=  -999,  (xc,yc,zc)  should  not  be  rotated  along  icid,  since 
(xc,yc,zc) are global coordinates. 
  When 
is 
*INCLUDE_TRANSFORM, (xc,yc,zc) is transformed. 
*INITIAL_VELOCITY_GENERATION 
1-182 (INTRODUCTION)
INTRODUCTION 
◦  Add 
of 
the 
time 
option 
ramping 
for 
*INITIAL_FOAM_REFERENCE_GEOMETRY.    The  solid  elements  with 
reference  geometry  and  ndtrrg > 0  will  restore  its  reference  geometry  in 
ndtrrg time steps. 
incorrect 
in 
velocity 
*INITIAL_VELOCITY_GENERATION,  and  rotational  velocity,  omega,  is 
not zero and *PART_INERTIA is also present. 
ICID.ne.0 
ndtrrg, 
initial 
steps, 
when 
◦  Fix 
◦  Add variable IZSHEAR in *INITIAL_STRESS_SECTION to initialize shear 
stress. 
◦  Fix  incorrect  initial  velocity  for  *INITIAL_VELOCITY  if  IRIGID = -2  and 
ICID > 0. 
◦  Fix incorrect NPLANE and NTHICK for *INITIAL_STRESS_SHELL when 
writing dynain for shell type 9. 
◦  Fix *INITIAL_STRAIN_SHELL output to dynain for shell types 12 to 15 in 
2D  analysis.    Write  out  strain  at  only  1  intg  point  if  INTSTRN = 0  in 
*INTERFACE_SPRINGBACK_LSDYNA  and  all  strains  at  all  4  intg  points 
if INTSTRN = 1 and nip = 4 in *SECTION_SHELL. 
the 
◦  Skip 
transformation  of 
ICID > 0  and 
*INCLUDE_TRANSFORM  is  used  to  transform  the  keyword  input  file 
with the *INITIAL_VELOCITY....  keyword.  Also echo warning message, 
KEY+1109, that the transformation will be skipped since icid is specified. 
◦  Fix  incorrect  transformation  of  *DEFINE_BOX  which  results  in  incorrect 
initial  velocities 
if 
initial velocities if the box is used in *INITIAL_VELOCITY. 
◦  Fixed *INITIAL_STRESS_DEPTH when used with 2D plane strain and ax-
isymmetric elements.  The prestress was being zeroed. 
◦  Improved  the  precision  of  the 
initial  deformation  calculation  for 
*INITIAL_FOAM_REFERENCE_GEOMETRY  in  the  single  precision  ver-
sion. 
◦  Fixed stress initialization (*INITIAL_STRESS_SECTION) for type 13 tet el-
ements.  The pressure smoothing was causing incorrect pressure values in 
the elements adjacent to the prescribed elements. 
◦  Add _SET option to *INITIAL_STRESS_SOLID for element sets. 
◦  Fix  bug 
in  3D  adaptivity 
*INITIAL_TEMPERATURE for adaptive parts. 
that  users 
so 
can  now  define 
•  Isogeometric Elements  
◦  The stability of the trimmed NURBS shell patches has been improved. 
◦  Add *LOAD_NURBS_SHELL to apply traction type loading directly on the 
surface of NURBS shell. 
◦  Users  can  use  the  PART  option  of  *SET_SEGMENT_GENERAL  to  define 
segment set of a NURBS patch.  The segment set will contain all segments 
of interpolated null shell elements. 
◦  *ELEMENT_SOLID_NURBS_PATCH:
INTRODUCTION 
  Isogeometric solid analysis implemented for MPP. 
  Isogeometric  solid  analysis  implemented  for  SMP  with  multiple 
CPUs, including consistency (ncpu < 0). 
  Activate user-defined materials for isogeometric solid. 
◦  *ELEMENT_SHELL_NURBS_PATCH: 
  Isogeometric shell analysis now implemented for SMP with multiple 
CPUs, including consistency (ncpu < 0). 
  Add a power iteration method to get the maximum eigen-frequency 
for each isogeometric element.  This will be  used to set a reasonable 
time step for trimmed elements. 
◦  *ELEMENT_SHELL_NURBS_PATCH: 
  Changed  the  way  of  projecting  the  results  from  isogeometric 
(NURBS) elements to the interpolation elements.  Now a background 
mesh, spanned over the locations of the integration points of the iso-
geometric  (NURBS)  elements  serves  as  basis  to  interpolate  results 
from  the  integration  points  to  the  centroid  of  the  interpolation  ele-
ments.  This change may lead to slightly different post-processing re-
sults in the interpolation elements. 
◦  Add support for trimmed NURBS to work in single precision.  Anyway, it 
is still recommended to use double precision versions for trimmed NURBS 
patches. 
◦  Add post-processing of strains and thickness for interpolation shells. 
•  *LOAD  
◦  Fixed  bugs  affecting  discrete  beam  elements  (ELFORM = 6)  when  used 
with staged construction.  Here, "dormant" refers to elements that have not 
on 
as 
yet 
*DEFINE_STAGED_CONSTRUCTION_PART. 
defined 
become 
active 
  Dormant  discrete  beams  could  still  control  the  timestep  and  attract 
mass-scaling, when they should not do so. 
  Dormant  discrete  beams  reaching  a  failure  criterion  defined  on  the 
*MAT card were deleted, when they should not be. 
  The  displacements  output    included 
displacements occurring while the elements were dormant.  Now, the 
output displacements are reset to zero at the moment the element be-
comes active.
INTRODUCTION 
◦  Fixed 
bug 
on 
*CONTROL_STAGED_CONSTRUCTION  had  been  left  blank,  and  Dy-
namic Relaxation was active, an error termination occurred. 
Construction: 
Staged 
FACT 
in 
if 
◦  Fixed bug:  *LOAD_GRAVITY_PART (and also gravity loading applied by 
*DEFINE_STAGED_CONSTRUCTION_PART)  was  failing  to  account  for 
non-structural  mass  when 
load:  NSM  on 
*SECTION_BEAM and MAREA on *SECTION_SHELL. 
calculating  gravity 
◦  Fixed  bug  in  *LOAD_VOLUME_LOSS:  inconsistent  results  when  run  in 
SMP parallel. 
◦  Fix bugs affecting *LOAD_SEGMENT_FILE: 
  Remove LOAD_SEGMENT_FILE file size limit (It used to be 200M). 
  Apply correct pressure on the shared boundary between processors. 
◦  Fix  GRAV = 1  in  *PART  which  was  not  were  not  working  correctly  with 
*LOAD_DENSITY_DEPTH.    Make  *LOAD_DENSITY_DEPTH  work  for 
Lagrangian 2D elements. 
◦  Fix 
insufficient 
memory 
error,SOL+659, 
when 
using 
*LOAD_ERODING_PART_SET with MPP. 
◦  Fix  incorrect  loading  when  using  *LOAD_ERODING_PART_SET  with 
BOXID defined. 
◦  Added *LOAD_SUPERPLASTIC_FORMING for implicit analysis. 
◦  *LOAD_SUPERPLASTIC_FORMING box option now works in MPP. 
•  *MAT and *EOS  
◦  *MAT_197 (*MAT_SEISMIC_ISOLATOR) could become unstable when the 
parameter DAMP was left at its default value.  A workaround was to input 
DAMP as a small value such as 0.05.   The timestep for *MAT_197 is now 
smaller than previously, irrespective of the DAMP setting, and the behav-
ior is now stable even if DAMP is left at the default. 
◦  Fixed bug: Timestep calculation was wrong for *MAT_089 solid elements.  
Response could be unstable especially for higher values of Poisson's ratio, 
e.g.  0.4. 
◦  Fixed  bug:  An  error  trap  was  wrongly  preventing  ELFORM = 15  for 
elements  with 
(*MAT_ARUP_ADHESIVE). 
  Wedge 
*MAT_169 
ELFORM = 15 are now permitted. 
◦  *MAT_172 (*MAT_CONCRETE_EC2): 
Note that items (1) and (2) below can lead to different results compared to 
previous versions of LS-DYNA. 
  (1)  The  number  of  potential  cracks  in  MAT_172  shell  elements  has 
been increased from 2 to 4.  MAT_172 uses a fixed crack model: once 
the first crack forms, it remains at the same fixed angle relative to the 
element  axes.    Further  cracks  can  then  form  only  at  pre-defined  an-
INTRODUCTION 
gles to the first crack.  Previously, only one further crack could form, 
at 90 degrees to the first crack.  Thus, if the loading direction subse-
quently  changed  so  that  the  principal  tension  is  at  45  degrees  to  the 
first  crack,  that  stress  could  exceed  the  user-defined  tensile  strength 
by a considerable margin.  Now, further cracks may form at 90, +45 
and -45 degrees to the first crack.  Although the maximum principal 
stress can  still exceed  the user-defined tensile strength, the "error" is 
much reduced.  There is an option to revert to the 2-crack model as in 
R9 (to do this, add 100 to TYPEC). 
  (2)  Add  element  erosion  to MAT_172.    This  change  may  lead  to  dif-
ferent  results  compared  to  previous  versions,  because  erosion  strain 
limits  are  now  added  by  default.    Elements  are  now  deleted  when 
crack-opening  strain  becomes  very  large,  or  the  material  is  crushed 
beyond the spalling limit.  Plastic strain in the rebar is considered too.  
Previously, these elements that have passed the point of being able to 
generate any stress to resist further deformation would remain in the 
calculation,  and  sometimes  showed  very  large  non-physical  defor-
mations  and  could  even  cause  error  terminations.    Such  elements 
would now be deleted automatically.  Default values are present for 
the erosion strains but these can be overridden in the input data, see 
new input fields ERODET, ERODEC, ERODER. 
  (3) New history variables 10,11,12 (maximum value so far of through-
thickness  shear  stress).    This  is  useful  for  checking  results  because 
MAT_172  cracks  only  in  response  to  in-plane  stress;  before  cracking 
occurs,  the  through-thickness  shear  capacity  is  unlimited.    The  data 
components are:  
Ex History Variable 10 - maximum out of 11 and 12  
Ex History Variable 11 - maximum absolute value of YZ shear stress  
Ex History Variable 12 - maximum absolute value of ZX shear stress  
These are in the element local axis system.  Note that these variables 
are  written  only  if  TYPESC  is  zero  or  omitted.    TYPESC  is  a  pre-
existing capability that requests a different type of shear check. 
  (4)  Fixed  bug.    Elastic  stiffness  for  MAT_172  beams  was  not  as  de-
scribed  in  the  manual,  and  the  axial  response  could  sometimes  be-
come unstable.  The bug did not affect shell elements, only beams. 
  (5) *MAT_172 can now handle models  with temperatures defined in 
Kelvin  (necessary  if  the  model  also  has  heat  transfer  by  radiation).  
*MAT_172 has thermally-sensitive material  properties hard-wired to 
assume  temperatures  in  Centigrade.    A  new  input  TMPOFF  in 
*MAT_172 offsets the model temperatures before calculating the ma-
terial properties. 
  (6) When the input parameter AGGSZ is defined, the maximum shear 
stress that can be transferred across closed cracks is calculated from a 
formula that has tensile strength and compressive stress as inputs.  In 
MAT_172, the tensile strength of concrete is reduced when compres-
INTRODUCTION 
sive damage has occurred .  Up to now, 
compressive  damage  was  therefore  influencing  the  maximum  shear 
across  cracks.    However,  the  Norwegian  standard  from  which  the 
shear formula is taken treats the tensile strength as a constant.  There-
fore, for the purpose of calculating the maximum shear stress across 
closed cracks only, the compressive damage effect is now ignored. 
  (7) Added capability for water pressure in cracks, for offshore appli-
cations.    The  water  pressure  is  calculated  from  the  depth  of  the  ele-
ment below the water surface (calculated from the z-coordinate).  The 
water pressure is applied as a compressive stress perpendicular to the 
plane of any crack in the element.  See new input fields WRO_G and 
ZSURF. 
◦  *MAT_119  (*MAT__GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM): 
Fixed bug in UNLOAD option 2.  The bug occurs if an unloading curve has 
been left zero (e.g.  LCIDTUR) while the corresponding loading curve was 
non-zero (e.g.  LCIDTR), and UNLOAD = 2.  Depending on the computer 
system, the symptoms could be harmless or the code could crash.  Now, if 
the unloading curve is left blank, it is assumed to be the same as the load-
ing curve i.e.  load and unload up and down the same curve.  That behav-
ior was already implemented for UNLOAD = 1. 
◦  Added Equation Of State 19 (*EOS_MURNAGHAN).  Used extensively for 
fluid modeling in SPH through Weakly-Compressible formulation, in con-
junction  with  SPH  formulations  15  (fluid  form)  and  16  (normalized  fluid 
form). 
◦  *MAT_ADD_FATIGUE: Added a new form of Basquin equation to define 
material's SN curve: LCID = -3: S = a*N^b, where a and b are material con-
stants. 
◦  Add  the  option  of  A0REF  for  *MAT_FABRIC.    That  allows  the  option  of 
using reference geometry to calculate A0 for the purpose of porosity leak-
age calculation. 
◦  Add optional parameter DVMIN for *MAT_ADD_PORE_AIR to define the 
min volume ratio change to trigger pore air flow analysis. 
◦  *DEFINE_HAZ_PROPERTIES: 
◦  Distance  of  shell  from  the  weld  center  is  treated  consistently  under  MPP 
and the shell material's yield stress is scaled properly. 
◦  *MAT_168 and *MAT_279: Fixed support for element erosion. 
◦  *MAT_092: Improved of implicit convergence for shells. 
◦  *MAT_224: Fixed bug where wrong shear modulus was used in EOS. 
◦  *MAT_270: Increased stability for thickness strain iterations for shells. 
◦  *MAT_240: Added support for cohesive shell formulation +/-29. 
◦  Scale  load  curve,  LCSRS,  of  *MAT_ADD_EROSION  when  used  with 
*INCLUDE_TRANSFORM.
INTRODUCTION 
◦  Fix 
incorrect 
using 
results 
*MAT_TABULATED_JOHNSON_COOK/*MAT_224  with  table  LCKT  de-
fined and the first abscissa value, temperature, is negative. 
table 
◦  Fix  spurious  element  deletion  when  using 
for  LCF 
when 
*MAT_TABULATED_JOHNSON_COOK/*MAT_224 
*MAT_TABULATED_JOHNSON_COOK_GYS/*MAT_224GYS. 
in 
and 
◦  Error terminate with message, KEY+1142, if *MAT_ADD_EROSION is ap-
plied  to  resultant  materials  28,116,117,118,130,139,166,170  and  98(with  1 
intg point). 
◦  Increase 
robustness 
of 
*MAT_033/*MAT_BARLAT_ANISOTROPIC_PLASTICITY for solids. 
◦  Fix 
input 
error 
when 
*MAT_ELASTIC_WITH_VISCOSITY_CURVE/*MAT_060c 
LCID = 0. 
using 
when 
◦  Fix  seg  fault  when  using  shell  type  15,  axisymmetric  volume  weighted, 
with *MAT_ADD_EROSION and also materials with equation-of-states. 
◦  Store computed yield strength as history variable #6 for *MAT_255. 
◦  Fix 
for 
inconsistency 
*MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY/*MAT_123  when 
ncpu < 0. 
◦  Include original volume output to dynain file for 2D analysis when materi-
als with an equation-of-state are used.  This is needed to compute the de-
formation gradient when initializing a run using the dynain file. 
◦  Fix  improper  stress  initialization  using  *INITIAL_STRESS_SHELL  via 
dynain for *MAT_018/*MAT_POWER_LAW_PLASTICITY with VP = 1.0. 
◦  Make 
for 
*MAT_170/*MAT_RESULTANT_ANISOTROPIC,  i.e.    with  material  coor-
dinate system using *DEFINE_COORDINATE_(OPTION). 
AOPT < 0 
work 
◦  Fix 
incorrect 
operation 
*MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY/*MAT_124 
*MAT_PLASTICITY_WITH_DAMAGE/*MAT_081/*MAT_082. 
TDEL 
of 
for 
and 
◦  Fix  incorrect  damping  when  using  *DAMPING_PART_STIFFNESS  for 
and 
*MAT_16/*MAT_PSEUDO_TENSOR 
*EOS_TABULATED_COMPACTION. 
◦  Fix  incorrect  computation  of  bulk  modulus  which  caused  complex  sound 
speed  error  when  using  *EOS_TABULATED/EOS_09  with  tabulated  in-
put. 
◦  Fix  moving  part  with  *MAT_220  during  dynamic  relaxation  when  veloci-
ties are initialized. 
◦  Fix 
for 
*MAT_065/*MAT_MODIFIED_ZERILLI_ARMSTRONG  for  shells  when 
VP = 1. 
convergence 
issue 
◦  Error  terminate  with  message,  KEY+1115,  if  _STOCHASTIC  option  is  in-
no 
for  materials 
10,15,24,81,98, 
voked 
123 
but 
or
INTRODUCTION 
*DEFINE_STOCHASTIC_VARIATION  or  *DEFINE_HAZ_PROPERTIES 
keyword is present in the input file. 
◦  Fix  spurious  error  termination  when  using  *DEFINE_HAZ_PROPERTIES 
with adpativity. 
◦  Fix 
incorrect 
results 
or 
seg 
fault 
for 
*MAT_FU_CHANG_FOAM/*MAT_083 if KCON > 0.0 and TBID.ne.0. 
◦  If SIGY = 0 and S = 0 in *MAT_DAMAGE_2/*MAT_105, set S = EPS1/200, 
where EPS1 is the first point of yield stress input or the first ordinate point 
of the LCSS curve. 
◦  Allow  *MAT_ENHANCED_COMPOSITE_DAMAGE/*MAT_054  failure 
mechanism to work together with *MAT_ADD_EROSION for shells. 
◦  Fix incorrect erosion behavior if *MAT_ADD_EROSION is used with fail-
for 
ure 
*MAT_123/*MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY. 
defined 
criteria 
◦  Implement *MAT_FHWA_SOIL/*MAT_147 for 2D analysis, shell types 13, 
14 and 15. 
◦  Implement 
scaling 
of 
failure 
strain 
for 
*MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY_STOCHASTIC/*
MAT_123_STOCHASTIC for shells. 
◦  Fix 
for 
*MAT_LINEAR_ELASTIC_DISCRETE_BEAM/*MAT_066  when  using 
damping with implicit (static) to explicit switching. 
behavior 
incorrect 
◦  Fixed  *MAT_FABRIC/*MAT_034  with  the  negative  unloading  curve  op-
tion.    When  searching  for  the  intersection  point  of  the  load  and  unload 
curves, and extrapolation of one of the curves was needed to find the inter-
section  point,  the  extrapolated  stress  was  calculated  incorrectly  causing 
unpredictable behavior. 
◦  Fixed fabric material forms 0 and 1 when used with a reference geometry.  
There were two problems, both occurring when there are mixed quad and 
triangular elements in the same block.  A flaw in the strain calculation was 
leading to possible NaN forces in the elements.  When a reference geome-
try  was  not  used,  the  forces  from  triangular  elements  in  mixed  element 
blocks were 2 times too high. 
◦  Added a new option for *MAT_SPOTWELD called FMODE.  The FMODE 
option  is  available  for  DMGOPT = 10, 11,  and  12.    When  the  failure  func-
tion  is  reached,  and  when  FMODE > 0.0  and < 1.0,  the  value  of  FMODE 
will determine if a weld will fail immediately, or will have damage initiat-
ed.    The  failure  function  may  include  axial,  shear,  bending  and  torsion 
terms.  If the sum of the squares of the shear and torsion terms divided by 
the  sum  of  the  square  of  all  terms  is  greater  than  FMODE,  then  the  weld 
will fail immediately.  Otherwise, damage will be initiated. 
◦  Enabled OPT = -1 on *MAT_SPOTWELD for brick elements which had not 
worked  previously.    Also,  fixed  TRUE_T  when  used  with  brick  element 
forms 0, 1, and -1.
INTRODUCTION 
◦  Fixed  spotwelds  with  DMGOPT = 12  by  removing  warning  STR+1327 
which made it impossible to set a small value of RS without triggering this 
warning, or without setting EFAIL smaller.  Setting EFAIL small however 
could lead to damage initiation by plastic strain when the user wanted on-
ly initiation by the failure function. 
◦  If DMGOPT = 10, 11, or 12 and EFAIL = 0, on *MAT_SPOTWELD, damage 
will  now  initiate  only  by  the  failure  function.    If  EFAIL > 0,  then  damage 
will  initiate  be  either  then  failure  function  or  when  plastic  strain  exceeds 
EFAIL.  Prior to this version, damage could initiate when plastic strain ex-
ceeds  zero  if  the  user  set  EFAIL = 0.    This  behavior  is  still  true  for 
DMGOPT = 0, 1, or 2, but no longer for DMGOPT = 10, 11, or 12. 
◦  Allow  solid  spot  welds  and  solid  spot  weld  assemblies  to  have  up  to  300 
points  in  the  running  average  that  is  used  to  smooth  the  failure  function.  
In other words, up to NF = 300 is possible. 
◦  Fixed a problem with  brick spot weld assemblies  when OPT = 0  failure is 
used  without  defining  any  weld  resultant  values.    Welds  were  being  im-
mediately deleted. 
◦  Added  new  PID  option  for  *DEFINE_SPOTWELD_FAILURE  (applies  to 
*MAT_SPOTWELD,  OPT = 10).    Changes  the  Card  3  input  for  static 
strength values to use part set ID’s rather than material ID’s. 
◦  Modified  shell  *MAT_214/*MAT_DRY_FABRIC  to  calculate  fiber  strains 
based on the current distance between the points where the fibers intersect 
with the element edges.  Previously, they were calculated from the rate-of-
deformation, but this was not as accurate as the new total strain measure. 
◦  Fixed  unit  scaling  for  GAMAB1  and  GAMAB2  on  *MAT_DRY_FABRIC.  
◦  Reworked 
We were incorrectly transforming them as stress. 
stress 
in 
*MAT_225/*MAT_VISCOPLASITC_MIXED_HARDENING  to  prevent  a 
divide by zero. 
update 
plastic 
the 
◦  Enabled *MAT_ADD_EROSION to be used with beams that have user de-
fined integration.  Memory allocation was fixed to prevent memory errors. 
◦  Fixed *MAT_106 when used with tshell form 5 or 6.  The elastic constants 
used in the assumed strain field were not reasonable. 
◦  Fix issue that could have led to problems using *MAT_054 (or *MAT_058 
or *MAT_158) in combination with TFAIL/TSIZE.gt.0.0 and damping. 
◦  *MAT_054 - *MAT_ENHANCED_COMPOSITE_DAMAGE:  
  Add  possibility  to  use  failure  criterion  in  *MAT_054  for  solids  in  a 
transversal  isotropic  manner.    It  is  assumed  that  the  material  1-
direction is the main axis and that the behavior in the 2-3 plane is iso-
tropic.  This feature is invoked by setting TI = 1 in *MAT_054. 
◦  *MAT_058 - *MAT_LAMINATED_COMPOSITE_FABRIC:
INTRODUCTION 
  Bugfix  for  shear  stiffness  behavior  in  *MAT_058  when  using  a  table 
definition  for  GAB  and  only  providing  stress-strain-curves  for  posi-
tive shear. 
  Bugfix  for  strain-rate  dependent  stiffness  behavior  in  *MAT_058 
when using a table definition for EA, EB or GAB under compressive 
loading. 
  Add  default  values  for  strengths  (XT,XC,YT,YC,SC)  1.e+16  for 
*MAT_058.  If no values for the strengths were defined, unpredictable 
things could have happened. 
◦  *MAT_138 - *MAT_COHESIVE_MIXED_MODE:  
  Store total mixed-mode and normal separation (delta_II & delta_I) on 
history  variables  1&2 
*MAT_COHESIVE_MIXED_MODE 
(*MAT_138).  This is only for post-processing and should not lead to 
any changes in the results. 
for 
◦  *MAT_157 - *MAT_ANISOTROPIC_ELASTIC_PLASTIC: 
  Add Tsai-Hill failure criterion (EXTRA = 2). 
  Allow 
strain-rate 
values 
dependent 
(XT,XC,YT,YC,ZT,ZC,SXY,SYZ,SZX) using *DEFINE_CURVE.  This is 
available for Tsai-Wu (EXTRA = 1) and Tsai-Hill. 
strength 
  Fixed  bug  in  using  *MAT_157  with  IHIS.gt.0  for  shells.    Thickness 
strain  update  d3  was  not  correct  and  plasticity  algorithm  may  have 
failed. 
  Add additional option to IHIS in *MAT_157 for SHELLs. 
  Now also the strength values (XT,XC,YT,YC,SXY) may be initialized 
via *INITIAL_STRESS_SHELL.  See variable IHIS and remarks in the 
User's Manual for details of initializing various blocks of material pa-
rameters. 
◦  *MAT_215 - *MAT_4A_MICROMEC: 
  Add  new  material  *MAT_215  that  is  a  micromechanical  material 
model that distinguishes between a fiber/inclusion and a matrix ma-
terial.    The  material  is  intended  for  anisotropic  composite  materials, 
especially  for  short  (SFRT)  and  long  fiber  thermoplastics  (LFRT).  
This model is available for shells, tshells and solids. 
◦  *MAT_225 - *MAT_VISCOPLASTIC_MIXED_HARDENING: 
  Fixed 
*MAT_225 
(*MAT_VISCOPLASTIC_MIXED_HARDENING)  when  using  a  table 
for LCSS together with kinematic hardening. 
bug 
in
INTRODUCTION 
◦  *MAT_261 - *MAT_LAMINATED_FRACTURE_DAIMLER_PINHO: 
*MAT_262 - *MAT_LAMINATED_FRACTURE_DAIMLER_CAMANHO: 
  Allow 
for 
table 
input 
for  mats 
261/262.Table  represents  fracture  toughness  vs.    element  length  vs.  
strain rate (shells, tshells, solids) 
mats 
toughness  values 
261/262 
fracture 
when 
bug 
in 
  Fixed 
together  with  RYLEN = 2 
using 
in 
*DAMPING_PART_STIFFNESS 
*CONTROL_ENERGY. 
  Correct shear failure behavior in *MAT_262.  This will most probably 
have no effect to any real application, but could be seen in very spe-
cial 1-element tests. 
◦  Changed 
storage 
*MAT_249 
(*MAT_REINFORCED_THERMOPLASTIC).   A  new variable  POSTV  con-
trols  which  variables  are  written  and  at  what  history  variable  location  in 
d3plot. 
variables 
history 
for 
of 
◦  *MAT_254  (*MAT_GENERALIZED_PHASE_CHANGE)  can  now  be  used 
with shell elements and thermal thick shells. 
◦  Added  flag  'EZDEF'  to  *MAT_249_UDFIBER.    In  this  case  the  last  row  of 
the deformation gradient is replaced by 0-0-1. 
damage 
limitation 
opt. 
◦  Add 
curve/table 
LCDLIM 
for 
*MAT_ADD_GENERALIZED_DAMAGE. 
◦  Add 
pre-defined 
damage 
tensors 
option 
PDDT 
to 
*MAT_ADD_GENERALIZED_DAMAGE. 
◦  *MAT_ADD_GENERALIZED_DAMAGE  now  works  for  solid  elements 
(only shells in R9). 
◦  Add optional failure criterion FFCAP to *MAT_100 with OPT = -1 or 0. 
◦  Enable *MAT_ADD_COHESIVE to be used in implicit analysis. 
◦  Add alternative version of *MAT_280 invoked by new flag on 1st card.  It 
is a physically based damage model with 4 new parameters. 
◦  Enable  *DEFINE_CONNECTION_PROPERTIES'  option  PROPRUL>=2  to 
be used with spotweld clusters, i.e.  not only 1 hex element but several (via 
*DEFINE_HEX_SPOTWELD_ASSEMBLY 
on 
*CONTROL_SPOTWELD_BEAM). 
RPBHX > 1 
or 
◦  Enable *MAT_ADD_EROSION to be safely used with material models that 
have  more  than  119  history  variables,  for  now  the  new  limit  is  169  (e.g.  
necessary for *MAT_157 with IHIS = 7). 
◦  Add  Tsai-Wu  failure  criterion  to  *MAT_157  for  solid  and  shell  elements 
invoked by EXTRA = 1 on card 6 and corresponding parameters on cards 8 
and 9. 
◦  Add viscoelastic option to *MAT_187 (SAMP-1).  Rate dependent Young's 
modulus and associated settings can be defined on new optional card 5. 
◦  Add new option IRNG for *DEFINE_STOCHASTIC_VARIATION to gov-
ern random number generation (deterministic or true random).
INTRODUCTION 
◦  Add  option  to  define  element  size  dependent  parameters  EN  and  SN  for 
*MAT_120 and *MAT_120_JC by setting them to negative values (curves). 
◦  Minor improvements for *MAT_252: Optional output of damage initiation 
information and more post-processing history variables. 
◦  If the first abscissa value of *MAT_224's failure strain curve LCG is nega-
tive, it is assumed that all abscissa values are natural logarithms of a strain 
rate. 
◦  Put *MAT_100_DA's "failure function" value to history variable 18. 
◦  Add  optional  in-plane  failure  strain  to  *MAT_169  (ARUP_ADHESIVE): 
new input parameter FSIP. 
◦  *MAT_USER_DEFINED_MATERIAL_MODELS now provides a few more 
variables  for  cohesive  elements,  i.e.    additional  arguments  in  subroutines 
umatXXc:  temperature,  element  size,  implicit  rejection  flag,  integration 
point identifier, and total number of integration points. 
◦  A  modified  version  of  the  3-parameter  Barlat  model  (*MAT_036)  is  intro-
duced  as  *MAT_EXTENDED_3-PARAMETER_BARLAT.    In  this  model, 
hardening  in  00,  45,  90,  biaxial  and  shear  can  be  specified  as  load  curves.  
Furthermore,  r-values  in  00,  45,  90,  biaxial  and  shear  can  be  specified  in 
terms of load curves vs plastic strain or constants.  This is an extension of 
hardening law 7 of the original 3-parameter Barlat model. 
version 
implicit 
◦  Improve 
of 
*MAT_098/*MAT_SIMPLIFIED_JOHNSON_COOK. 
◦  *MAT_181/*MAT_SIMPLIFIED_RUBBER/FOAM  is  now  supported  for 
2D implicit simulations. 
◦  Fixed  issue  in  which  *MAT_WINFRITH_CONCRETE  wrote  d3crack  data 
too frequently. 
◦  *EOS_JWL  now  has  an  AFTERBURN  option.    This  adds  afterburn  energy 
to the EOS, where the energy can be added at a constant or linear rate, or 
can be added according to Miller's extension. 
◦   
◦  *MAT_084 
(*MAT_WINFRITH_CONCRETE)  with  predefined  units 
(CONM < 0) is now transformed correctly with *INCLUDE_TRANSFORM. 
◦  User-defined  materials  for  Hughes-Liu  beams  can  now  be  used  with  im-
plicit analysis by defining the appropriate tangent modulus in the supplied 
routine urtanb. 
◦  User-defined cohesive materials can now be used with implicit analysis by 
defining the appropriate tangent stiffness. 
◦  *MODULE for user-defined materials and other user-defined capabilities: 
  A  new  command  line  option  "module = filename"  is  added  to  load 
one  module  file  without  changing  the  input  deck.    It  provides  back 
compatibility to input deck without the MODULE keywords. 
  The  system  paths  defined  in  LD_LIBRARY_PATH  are  also  included 
for searching module files for those filenames start with "+".
INTRODUCTION 
◦  Add 
shell 
implementation 
to 
*MAT_277 
(*MAT_ADHESIVE_CURING_VISCOELASTIC). 
◦  Add *MAT_278 for carbon fiber prepreg compression forming simulation.  
This material model is available for both solid and shell formulations. 
◦  Add  *MAT_293  non-orthogonal  material  model  for  carbon  fiber  prepreg 
forming simulation.  This material model is only available for shell formu-
lations. 
◦  *MAT_260A: 
  Extend *MAT_260A to include solid elements. 
  Add  a  new  option  XUE  for  Xue's  fracture  criteria/theory  for 
*MAT_M260A (solid elements only). 
◦  *MAT_260B: 
  Set default values for P's and G's in *MAT_260B. 
  Add  a  length  scale  to  the  fracture  limit.    The  fracture  limit  strongly 
depends on the length scale in the measurement. 
  Add a new fracture criterion to *MAT_260B (Xue and Wierzbicki, Int.  
J.  solids and Structures 46 (2009) 1423-1435).  When the option XUE 
is activated, an additional card is needed, for example: 
  $      ef0      plim         q      gama         m 
        0.70      925.7  0.970       0.296     2.04 
◦  *MAT_037: 
  Improve  *MAT_037  with  negative  R  value  in  implicit  calculation.  
The modification will allow the implicit method stress calculation to 
be more accurate. 
  Add a new option NLP2 to calculate formability index in *MAT_037.  
The  previous  method  (option  NLP_FAILURE)  was  based  on  the  ef-
fective strain method, which assumes that necking happens at one in-
stant.    In  fact,  it  might  happen  over  a  longer  process.    The  new 
method calculates the damage accumulation. 
◦  Add  *MAT_165B  (*MAT_PLASTIC_NONLINEAR_KINEMATIC_B)  for 
shells and solids. 
•  MPP  
◦  Fix the report of decomp balance (shown as "Normalized element costs as-
signed  during  decomposition"  in  the  d3hsp  file),  which  was  broken  in 
r109760 
◦  MPP decomposition has not been properly balanced since r112652 due to a 
bug in that revision
INTRODUCTION 
◦  Fix  MPP 
SYNC 
error  due 
to 
inconsistent 
summation 
in 
*CONTACT_SLIDING_ONLY_PENALTY. 
◦  Allow real values as the scale multipliers for "memory=" on the command 
line.  For example, "memory = 2.5G memory2 = 1.1G" and the like. 
◦  MPP: fix support for nlq setting in *CONTROL_SOLUTION which was not 
being honored on processors other than 0. 
◦  Significant  improvements  in  MPP  groupable  routines  for  FORMING  con-
tact. 
◦  MPP:  increase  contact  release  distance  for  SINGLE_SURFACE  contacts  in 
the case of a node coming into contact with a solid element.  The previous 
interpretation  was  releasing  when  the  contact  penetration  was  0.5*solid 
thickness,  but  now  when  the  node  passes  below  the  solid  surface  by 
0.5*solid thickness (which is different by the half thickness of the slave ma-
terial, in the case of a shell slave node). 
◦  MPP: fix for viscous damping in automatic tiebreak contact. 
◦  Implement  new  bucket  sort  based  extent  testing  for  MPP  single  surface 
contact. 
◦  Added 
MPP 
support 
for 
*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_LUBRICATION. 
◦  Fixed  *CONTROL_MPP_PFILE  so  that 
it  honors  ID  offsets  from 
*INCLUDE_TRANSFORM  for  parts,  part  sets,  and  contact  IDs  referenced 
in "decomp { region {" specifications. 
◦  Furthermore, such a region can contain a "local" designation, in which case 
the decomposition of that region will be done in the coordinate system lo-
cal to the include file, not the global system.  For example: 
◦  *CONTROL_MPP_PFILE decomp { region {  partset 12 local c2r 30 0 -30 0 1 
0 1 0 0 } } would apply the c2r transformation in the coordinate system of 
the include file, which wasn't previously possible.  The local option can be 
useful even if there are no such transformations, as the "cubes" that the de-
composition  uses  will  be  oriented  in  the  coordinate  system of  the  include 
file, not the global system. 
◦  Furthermore,  the  following  decomposition  related  keywords  now  have  a 
_LOCAL option, which has the same effect: 
  *CONTROL_MPP_DECOMPOSITION_PARTS_DISTRIBUTE_LOCA
L 
  *CONTROL_MPP_DECOMPOSITION_PARTSET_DISTRIBUTE_LO
CAL 
  *CONTROL_MPP_DECOMPOSITION_ARRANGE_PARTS_LOCAL 
  *CONTROL_MPP_DECOMPOSITION_CONTACT_DISTRIBUTE_L
OCAL 
◦  MPP job performance profiles are output to both .csv and .xy files. 
•  OUTPUT
INTRODUCTION 
◦  Fix  for  writing  d3plot  file  when  individual  output  states  exceed  8GB  in 
single precision 
◦  Added  new  option  *INTERFACE_SPRINGBACK_EXCLUDE  to  exclude 
selected portions from the generated dynain file. 
◦  Add a new option to *INTERFACE_COMPONENT_FILE to output only 3 
degrees of freedom to the file even if the current model has 6. 
◦  Fix  missing  plastic  strain 
*DATABASE_EXTENT_BINARY 
*INTERFACE_SPRINGBACK. 
tensors 
is 
in  d3plot  when  STRFLG 
set 
INTSTRN = 1 
and 
in 
in 
◦  Fix  no  output  to  bndout  when  run  with  q = remap  even  though  the  key-
word  *DATABASE_BNDOUT  was  present  in  the  remap  run  but  was  not 
present in the initial run. 
◦  Fix  d3plot  output  frequency  which  was  different  from  the  dt  specified  in 
is 
*DATABASE_BINARY_D3PLOT  when  *CONTACT_AUTO_MOVE 
used. 
◦  Fix stress output to elout for solid elements which was in the global coor-
in 
in 
coordinates  when  CMPFLG = 1 
dinates 
*DATABASE_EXTENT_BINARY 
*DATABASE_ELOUT. 
OPTION1 > 0 
instead 
local 
and 
of 
◦  Fix  incorrect  mass  properties  for  solids  in  ssstat  file  when  using 
*DATABASE_SSSTAT_MASS_PROPERTY. 
◦  Fix  seg 
fault  during  writing  of  dynain 
in 
*INTERFACE_SPRINGBACK 
in 
*DATABASE_EXTENT_BINARY and the *DATABASE_EXTENT_BINARY 
comes after *INTERFACE_SPRINGBACK. 
STRFLG.ne.0 
INSTRN = 1 
and 
file 
if 
◦  If HYDRO is nonzero in *DATABASE_EXTENT_BINARY, LS-PrePost will 
now  combine  the  solid  and  shell  internal  energy  densities  when  fringing 
'Internal Energy Density' in the Misc menu. 
◦  By  putting  SIGFLG/EPSFLG = 3  in  *DATABASE_EXTENT_BINARY,  the 
stresses and plastic trains are excluded not only for shell elements but also 
for solids.  This applies to d3plot and d3eigv. 
◦  Added  new  file  option  *DATABASE_BINARY_INTFOR_FILE  to  define 
interface file name. 
◦  Fixed 
legend 
in 
bndout 
in 
the 
case 
of  multiple 
*BOUNDARY_PRESCRIBED_MOTION_SET_ID. 
◦  Fix 
d3part 
corrupt 
data 
*DATABASE_EXTENT_BINARY. 
◦  Fixed the legend of ssstat in binout. 
◦  Added  *DATABASE_EXTENT_SSSTAT_ID.   The  subsystem  id  will  be  in-
DECOMP = 4 
caused 
by 
in 
cluded in the ASCII ssstat file. 
◦  Fixed 
bug 
*CONTROL_OUTPUT. 
in 
stbout 
(seatbelt 
output) 
if  NEWLEG = 0 
in 
◦  Fixed bug in which DECOMP = 2 corrupted d3part. 
◦  Fixed d3plot bug if dynamic relaxation was activated in the input deck.
INTRODUCTION 
◦  Added  another  digit  for  coordinates  in  *NODE  in  dynain,  e.g.,  what  was 
written as 0.999266236E+00 is now written as 9.992662368E+00. 
◦  Added  *DATABASE_EXTENT_BINARY_COMP  for  alternative  (simpler) 
control of output to d3plot and d3eigv. 
  Output control flags: 0-no 1-yes 
  IGLB : Global data 
  IXYZ : Current coordinate 
  IVEL : Velocity 
  IACC : Acceleration 
  ISTRS: 6 stress data + plastic strain 
  ISTRA: 6 strain data 
  ISED : Strain energy density 
command 
regular 
This 
*DATABASE_EXTENT_BINARY  but  will  disable  most  of  the  options  in 
the latter, including output of extra history variables. 
combination  with 
can  be  used 
in 
◦  Bugfix:  *DATABASE_TRACER  without  the  optional  NID  parameter  was 
read  incorrectly  when  used  with  *INCLUDE_TRANSFORM,  but  is  now 
fixed 
◦  Fixed incomplete output from Windows version of LS-DYNA.  This affect-
curvout 
(*DATABASE_TRACER_DE) 
demtrh 
and 
ed 
(*DATABASE_CURVOUT). 
•  Restarts 
◦  Enable definition of sensors in full restarts. 
◦  For a small restart in MPP, the value of "memory=" (M1) needed for each 
processor is stored in the dump files.  This is the minimum requirement to 
read back the model info.  If the value of "memory2=" (M2) is specified on 
the command line, the code will take the maximum of M1 and M2. 
input  when 
error 
*INITIAL_VELOCITY_GENERATION 
*CHANGE_VELOCITY_GENERATION together in a full deck restart. 
using 
and 
structured 
during 
◦  Fix 
input 
◦  Fix incorrect full deck restart analysis if initial run was implicit and the full 
deck restart run is explicit.  This affects MPP only. 
◦  Fix insufficient tying of nodes when doing full deck restart and the contact 
is newly added to the restart involving newly added parts.  This applies to 
SMP contact only. 
◦  Fix  incorrect  velocity  initialization  for  SMP  full  deck  restart  when  using 
and 
*INITIAL_VELOCITY_GENERATION 
*INITIAL_VELOCITY_GENERATION_START_TIME. 
◦  Fix incorrect initialization of velocities for SMP full  deck restart when us-
ing  *CHANGE_VELOCITY_OPTION  &  *INITIAL_VELOCITY_OPTION.
INTRODUCTION 
Velocities of existing parts defined by *STRESS_INITIALIZATION should 
not be zeroed. 
◦  Fix *CHANGE_CURVE_DEFINITION for curve specifying d3plot output. 
◦  Fixed bug in full deck restart if the new mesh has different part numbers. 
•  *SENSOR 
◦  Fix 
a 
bug 
for 
*CONSTRAINED_JOINT_STIFFNESS,  that  was  triggered  when  the  force 
refers to a local coordinate system. 
*SENSOR_JOINT_FORCE 
regarding 
◦  Add the option of "ELESET" to *SENSOR_CONTROL to erode elements. 
◦  Add the option of NFAILE to *SENSOR_DEFINE_MISC to track number of 
eroded elements. 
◦  Fix  a  bug  that  was  triggered  when  using  a  sensor  to  control  spotwelds.  
The  bug  was  triggered  when  the  spotweld-connected  nodal  pairs  happen 
to belong to more than 1 core (MPP only). 
◦  Add  FAIL  option  to  *SENSOR_DEFINE_ELEMENT  to track  the  failure  of 
element(s). 
◦  Fix a bug related to *SENSOR_DEFINE_FUNCTION when there are more 
than 10 sensor definitions. 
◦  Effect  of  TIMEOFF 
TYPE = PRESC-ORI. 
◦  *SENSOR_CONTROL 
in  *SENSOR_CONTROL 
is 
implemented 
for 
can 
be 
used 
to 
control 
*BOUNDARY_PRESCRIBED_ORIENTATION_RIGID. 
◦  Add optional filter id to SENSORD of *DEFINE_CURVE_FUNCTION. 
◦  Enable 
*CONSTRAINED_JOINT_..._LOCAL 
to  be  monitored  by 
*SENSOR_DEFINE_FORCE. 
◦  Allow  moments 
in  SPCFORC  and  BNDOUT 
to  be 
tracked  by 
*SENSOR_DEFINE_FORCE. 
◦  Fix  *SENSOR_CONTROL  using  TYPE=“PRESC-MOT”  which  was  not 
switching at all. 
•  SPG (Smooth Particle Galerkin) 
◦  MPP  is  ready  in  3D  SPG  fluid  particle  stabilization  (ITB = 1  &  2  in 
*SECTION_SOLID_SPG). 
◦  Added one SPG control parameter (itb = 2) for semi-brittle fracture analy-
sis.  In comparison to itb = 0 or itb = 1, itb = 2 is more efficient in modeling 
the  fragmentation  and  debris  in  semi-brittle  fracture  analysis  such  as  im-
pact and penetration in concrete materials. 
◦  Fixed a bug related to E.O.S.  in SPG. 
◦  Removed some temporary memory allocations to improve efficiency. 
◦  Changed  the  sequence  of  SPG  initialization  so  that  all  state  variables  are 
properly initialized.
INTRODUCTION 
◦  Subroutines were developed for SPG failure analysis with thermal effects.  
Both explicit and implicit (diagonal scaled conjugate gradient iterative on-
ly)  SPG  thermal  solvers  are  available  in  SMP  version  only.    However, 
thermal effect is applied only on material properties, which means thermal 
induced deformation (i.e., thermal strain or thermal expansion) is not cur-
rently included. 
◦  Modified *MAT_072R3 for SPG method in concrete applications. 
◦  Fixed a bug for SPG method in using continuum damage mechanics.  (ID-
AM = 0). 
◦  Added  the  “fluid  particle  algorithm”  (itb = 1)  to  SPG  method.    This  algo-
rithm  is  implemented  in  R10.0  as  an  alternative  to  the  (itb = 0)  option  in 
previous version to enhance the numerical stability for SPG method.  Users 
are recommended to use this new option for their ductile failure analysis. 
•  SPH (Smooth Particle Hydrodynamics) 
◦  Add ITHK flag in *CONTROL_SPH, card 3.  If flag is set to 1, the volume 
of the SPH particles is used to estimate a node thickness to be employed by 
contacts. 
  Affects 
*AUTOMATIC_NODES_TO_SURFACE 
and 
*CONTACT_2D_NODE_TO_SOLID. 
  The thickness calculated by ITHK = 1 is used only if SST or OFFD are 
set to zero in the contact cards definitions. 
◦  Add SOFT = 1 option to *CONTACT_2D_NODE_TO_SOLID.  This should 
help obtain reasonable contact forces in axisymmetric simulations.  Default 
penalty PEN is 0.1 when SOFT = 1. 
◦  Implemented  non-reflecting  boundary  conditions  for  SPH  using  a  new 
keyword *BOUNDARY_SPH_NON_REFLECTING. 
◦  Bug  fix  for  renormalized  SPH  formulations  with  symmetry  planes.    The 
renormalization was slightly incorrect in the vicinity of symmetry planes. 
◦  Density  smoothing  in  SPH  formulations  15  and  16  is  now  material  sensi-
tive.  The smoothing only occurs over neighbors of the same material. 
◦  Resolved an MPP bug in SPH total Lagrangian formulations (FORM = 7/8) 
which  was  causing  strain  concentrations  at  the  interfaces  between  CPU 
zones. 
◦  SPH total Lagrangian (FORM = 7/8) in SMP was pretty much serial, hence 
much  slower  than  forms  0  or  1.    SPH  with  FORM  7  and  8  now  scales 
properly. 
◦  Added support for FORMs 0/1 in axisymmetric.  Until now, renormaliza-
tion was always active (equivalent to FORM = 1) which can be problematic 
for very large deformations or material fragmentation. 
◦  Improved tracer particles output for SPH: Use normalized kernel function 
for interpolation between particles.
INTRODUCTION 
◦  Implemented enhanced fluid flow formulations (FORMs 15/16) with pres-
sure smoothing. 
◦  Recode  SPH  neighborhood  search  algorithm  to  reduce  the  memory  re-
quirement and produce consistent results from MPP and HYBRID code. 
◦  *DEFINE_ADAPTIVE_SOLID_TO_SPH now reports both active and inac-
tive adaptive SPH particles in the fragment file sldsph_frag.  This file gives 
a report of nodal mass, coordinates, and velocities. 
◦  MPP now supports: 
  SPH type 3 inflow 
  Multiple *BOUNDARY_SPH_FLOW 
  Bulk viscosity option for SPH 
◦  Sort  SPH  by  part  and  then  node  ID  to  ensure  consistent  results  while 
changing order of input files. 
◦  *DEFINE_SPH_TO_SPH_COUPLING: 
  Corrected  the  SPH  sphere  radius  (half  of  the  particles  distance)  for 
node to node contact detecting algorithm. 
  Updated masses for SPH node to node  coupling with damping  con-
tact force option. 
  Added a new option (Soft = 1) for SPH to SPH coupling: contact stiff-
ness comes from particles masses and time step for softer contact. 
◦  *DEFINE_ADAPTIVE_SOLID_TO_SPH: 
  Updated temperature transfer (from solid elements to SPH particles) 
when  converting  solid  elements  into  SPH  particles  with  ICPL = 1, 
IOPT = 0. 
  Bug fixed when part ID for newly generated SPH particles is smaller 
than the original SPH part ID. 
  Introduced a new pure thermal coupling between SPH part and solid 
parts with ICPL = 3 and IOPT = 0 option (no structural coupling pro-
vided). 
  Added a thermal coupling conductivity parameter CPCD.  Applies to 
ICPL = 3 option. 
  Normalized the nodal temperatures for the corner SPH particles with 
ICPL = 3 and IOPT = 0 option (MPP only). 
  Extended  ICPL = 3  and  IOPT = 0  option  to  Lagrangian  formulation 
(form = 7, 8). 
◦  *BOUNDARY_SPH_SYMMETRY_PLANE: 
  Added in an error message if TAIL and HEAD points are at the same 
location.
INTRODUCTION 
◦  *CONTACT_2D_NODE_TO_SOLID: 
  Added a variable OFFD to specify contact offset. 
◦  Added a new option IEROD = 2 in *CONTROL_SPH in which SPH parti-
cles that satisfy a failure criterion are totally eactivated and removed from 
domain  interpolation.    This  is  in  contrast  to  IEROD = 1  option  in  which 
particles are partially deactivated and only stress states are set to zero. 
◦  Added  *MAT_SPH_VISCOUS  (*MAT_SPH_01)  for  fluid-like  material  be-
havior with constant or variable viscosity.  Includes a Cross viscosity mod-
el. 
◦  Output strain rates for SPH particles to d3plot, d3thdt, and sphout file. 
◦  Added  support  of  *MAT_ADD_EROSION,  including  GISSMO  and  DIEM 
damage, for SPH particles. 
◦  Echo failed SPH particles into d3hsp and messag file. 
◦  *DEFINE_SPH_INJECTION: 
  Changed the method of generating SPH particles.  SPH particles will 
be  generated  based  on  the  injection  volume  (injection  area*injection 
velocity*dt)*density  from  the  material  model,  resulting  in  more  con-
sistent particle masses and particle distribution. 
  Offset injecting distance inside each cycle so that outlet distance will 
be consistent for different outlet SPH layers. 
  Corrected mass output in d3hsp. 
•  Thermal Solver  
◦  Modify  the  thermal  solver  routines  so  they  return  instead  of  terminating, 
so that *CASE works properly. 
◦  *MAT_THERMAL_USER_DEFINED: Fixed bug in element numbering for 
IHVE = 1. 
◦  Accept 
load 
in 
*CONTROL_THERMAL_TIMESTEP.  As usual if a negative integer num-
ber is given its absolute value refers to the load curve id. 
for  dtmin,  dtmax  and  dtemp 
curve 
input 
◦  The  temperature  results  for  the  virtual  nodes  of  thermal  thick  shells  are 
now  accounted  for  in  *LOAD_THERMAL_D3PLOT.    For  the  mechanics-
only simulation thermal thick shells have to be activated. 
◦  New contact type for thermal solver that models heat transfer from and to 
a shell edge onto a surface (*CONTACT_..._THERMAL with ALGO > 1): 
  Shells have to be thermal thick shells. 
  Shells are on the slave side. 
  So far only implemented for SMP. 
  Includes support for quads and triangles.
INTRODUCTION 
◦  New keyword *BOUNDARY_THERMAL_WELD_TRAJECTORY for weld-
ing of solid or shell structures. 
  Keyword  defines  the  movement  of  a  heat  source  on  a  nodal  path 
(*SET_NODE). 
  Orientation given either by vector or with a second node set. 
  Works for coupled and thermal only analyses. 
  Allows for thermal dumping. 
  Different equivalent heat source descriptions available. 
  Can also be applied to tshells and composite shells. 
  Weld torch motion can be defined relative to the weld trajectory. 
◦  Solid element formulation 18 now supports thermal analysis. 
◦  Thermal solver now supports the H8TOH20 option of *ELEMENT_SOLID.  
This  includes  support  of  *INITIAL_TEMPERATURE  condition  for  the  ex-
tra 12 nodes generated by H8TOH20. 
◦  Thermal solver now supports the H8TOH27 option of *ELEMENT_SOLID. 
◦  Explicit Thermal Solver 
  *CONTROL_EXPLICIT_THERMAL_SOLVER:  Implement  an  explicit 
thermal solver and adapt it to support multi-material ALE cases. 
  *CONTROL_EXPLICIT_THERMAL_PROPERTIES:  Enter 
thermal 
properties for the explicit thermal solver. 
  *CONTROL_EXPLICIT_THERMAL_CONTACT:  Implement  a  ther-
mal contact for the explicit thermal solver. 
  *CONTROL_EXPLICIT_THERMAL_ALE_COUPLING:  Implement  a 
thermal coupling between ALE and Lagrangian structures for use by 
the explicit thermal solver. 
  *CONSTRAINED_LAGRANGE_IN_SOLID_EDGE:  For  the  explicit 
thermal ALE coupling, allow the heat transfer through the shell edges 
if _EDGE is added to *CONSTRAINED_LAGRANGE_IN_SOLID. 
  *CONSTRAINED_LAGRANGE_IN_SOLID:  For  the  explicit  thermal 
solver,  add  work  due to  friction  to  the  enthalpies  of  ALE  and  struc-
ture 
with 
*CONSTRAINED_LAGRANGE_IN_SOLID (CTYPE = 4). 
elements 
coupled 
  *CONTROL_EXPLICIT_THERMAL_INITIAL:  Initialize  the  tempera-
tures for the explicit thermal solver. 
  *CONTROL_EXPLICIT_THERMAL_BOUNDARY: Control boundary 
temperatures for the explicit thermal solver. 
  *CONTROL_EXPLICIT_THERMAL_OUTPUT:  Output  the  tempera-
tures at element centers for the explicit thermal solver. 
  *DATABASE_PROFILE:  For  the  explicit  thermal  solver,  output  tem-
perature profiles. 
•  Miscellaneous
INTRODUCTION 
◦  *INITIAL_LAG_MAPPING:  Implement  a  3D  to  3D  lagrangian  mapping 
and map the nodal temperatures. 
◦  *CONTROL_REFINE_SHELL  and  *CONTROL_REFINE_SOLID:  Add  a 
parameter MASTERSET to call a  set of nodes to flag element edges along 
which new child nodes are constrained. 
◦  *BOUNDARY_PRESCRIBED_MOTION_SET_SEGMENT:  Add  DOF = 12 
to apply velocities in local coordinate systems attached to segments. 
◦  Fixed 
bug 
when 
occurring 
non-zero 
*DAMPING_PART_STIFFNESS, 
using 
*PART_COMPOSITE,  AND  the  MIDs  referenced  by  the  different  integra-
tion  points  have  different  material types.   Symptoms  could  include  many 
types  of  unexpected  behavior  or  error  termination,  but  in  other  cases  it 
could be harmless. 
has 
defined 
a 
AND 
part 
is 
◦  *DAMPING_FREQUENCY_RANGE  (including  _DEFORM  option):  Im-
proved  internal  calculation  of  damping  constants  such  that  the  level  of 
damping more accurately matches the user-input value across the whole of 
the frequency range FLOW to FHIGH.  As an example, for CDAMP = 0.01, 
FLOW = 1  Hz  and  FHIGH = 30  Hz,  the  actual  damping  achieved  by  the 
previous algorithm varied between 0.008 and 0.012 (different values at dif-
ferent  frequencies  between  FLOW  and  FHIGH),  i.e.    there  were  errors  of 
up  to  20%  of  the  target  CDAMP.    With  the  new  algorithm,  the  errors  are 
reduced to 1% of the target CDAMP.  This change will lead to some small 
differences  in  results  compared  to  previous  versions  of  LS-DYNA.    Users 
wishing to retain the old method for compatibility with previous work can 
do this by setting IFLG (7th field on Card 1) to 1. 
in 
the 
Part 
included 
◦  Fixed bug that could cause unpredictable symptoms if Nodal Rigid Bodies 
by 
were 
or 
*DAMPING_FREQUENCY_RANGE 
*DAMPING_FREQUENCY_RANGE_DEFORM.    Now,  the  _DEFORM  op-
tion 
Set  while 
*DAMPING_FREQUENCY_RANGE (non _DEFORM option) damps them. 
◦  Fixed bug in *PART_COMPOSITE: if a layer had a very small thickness de-
fined, such as 1E-9 times the total thickness, that layer would be assigned a 
weighting factor of 1 (it should be close to zero). 
ignores  NRBs 
referenced 
silently 
Part 
the 
Set 
in 
◦  Fix errors in implementation of *DEFINE_FILTER type CHAIN. 
◦  Fix  for  *INTERFACE_LINKING_LOCAL  when  LCID  is  used.    During 
keyword processing, the LCID value was not properly converted to inter-
nal numbering. 
◦  Switch coordinates in keyword reader to double precision. 
◦  Change "Warning" to "Error" for multiply defined materials, boxes, coordi-
nate systems, vectors, and orientation vectors.  The check for duplicate sec-
tion  IDs  now  includes  the  element  type  and  remains  a  warning  for  now, 
because  SPH  is  still  detected  as  a  SOLID.    Once  that  is  straightened  out, 
this should be made an error.
INTRODUCTION 
◦  Add  "TIMESTEP"  as  a  variable  for  *DEFINE_CURVE_FUNCTION.    This 
variable holds the current simulation time step. 
◦  Fix 
a 
bug 
in 
*DEFORMABLE_TO_RIGID_AUTOMATIC.    (Fields  3  to  8  are  now  ig-
nored.) 
CODE = 5 
case 
the 
for 
of 
◦  Issue error message and terminate the simulation when illegal ACTION is 
used for *DEFINE_TRANSFORM. 
◦  Add  option  of  POS6N  for  *DEFINE_TRANSFORM  to  define  transfor-
mation with 3 reference nodes and 3 target nodes. 
◦  Fix  a  bug  that  can  occur  when  adaptive  elements  are  defined  in  a  file  in-
cluded by *INCLUDE_TRANSFORM. 
◦  Merge  *DEFORMABLE_TO_RIGID_AUTOMATIC  cards  if  they  use  the 
same  switch  time.    This  dependency  of  results  on  the  order  of  the  cards 
and also gives better performance. 
◦  If  *SET_PART_OPTION  is  used,  a  "group_file"  will  be  created  which  can 
be read into LS-Prepost (Model > Groups > Load) for easy visualization of 
part sets. 
◦  Forces on *RIGIDWALL_GEOMETRIC_CYLINDER can now be subdivid-
ed into sections for output to rwforc.  This gives a better idea of the force 
distribution along the length of the cylinder.   See the variable NSEGS. 
◦  Added 
the 
keywords 
*DEFINE_PRESSURE_TUBE 
and 
*DATABASE_PRTUBE for simulating pressure tubes in pedestrian crash. 
◦  Fix  non-effective  OPTIONs  DBOX,  DVOL,  DSOLID,  DSHELL,  DTSHELL, 
DSEG for *SET_SEGMENT_GENERAL to delete segments. 
◦  Fix  incorrect  transformation  of  valdmp  in  *DAMPING_GLOBAL  with 
*INCLUDE_TRANSFORM. 
◦  Make *SET_NODE_COLLECT work together with *NODE_SET_MERGE. 
◦  Fixed bug in adaptivity for *INCLUDE_TRANSFORM if jobid is used. 
◦  Bugfix: *INTERFACE_SSI with blank optional card is now read in correct-
ly. 
MATERIAL MODELS 
Some of the material models presently implemented are: 
•  elastic, 
•  orthotropic elastic, 
•  kinematic/isotropic plasticity [Krieg and Key 1976], 
•  thermoelastoplastic [Hallquist 1979], 
•  soil and crushable/non-crushable foam [Key 1974], 
•  linear viscoelastic [Key 1974],
INTRODUCTION 
•  Blatz-Ko rubber [Key 1974], 
•  high explosive burn, 
•  hydrodynamic without deviatoric stresses, 
•  elastoplastic hydrodynamic, 
•  temperature dependent elastoplastic [Steinberg and Guinan 1978], 
•  isotropic elastoplastic, 
•  isotropic elastoplastic with failure, 
•  soil and crushable foam with failure, 
•  Johnson/Cook plasticity model [Johnson and Cook 1983], 
•  pseudo TENSOR geological model [Sackett 1987], 
•  elastoplastic with fracture, 
•  power law isotropic plasticity, 
•  strain rate dependent plasticity, 
•  rigid, 
•  thermal orthotropic, 
•  composite damage model [Chang and Chang 1987a 1987b], 
•  thermal orthotropic with 12 curves, 
•  piecewise linear isotropic plasticity, 
•  inviscid, two invariant geologic cap [Sandler and Rubin 1979, Simo et al, 1988a 
•  1988b], 
•  orthotropic crushable model, 
•  Mooney-Rivlin rubber, 
•  resultant plasticity, 
•  force limited resultant formulation, 
•  closed form update shell plasticity, 
•  Frazer-Nash rubber model, 
•  laminated glass model, 
•  fabric, 
•  unified creep plasticity, 
•  temperature and rate dependent plasticity, 
•  elastic with viscosity, 
•  anisotropic plasticity,
INTRODUCTION 
•  user defined, 
•  crushable cellular foams [Neilsen, Morgan, and Krieg 1987], 
•  urethane foam model with hysteresis, 
and some more foam and rubber models, as well as many materials models for springs 
and  dampers.    The  hydrodynamic  material  models  determine  only  the  deviatoric 
stresses.  Pressure is determined by one of ten equations of state including: 
•  linear polynomial [Woodruff 1973], 
•  JWL high explosive [Dobratz 1981], 
•  Sack “Tuesday” high explosive [Woodruff 1973], 
•  Gruneisen [Woodruff 1973], 
•  ratio of polynomials [Woodruff 1973], 
•  linear polynomial with energy deposition, 
•  ignition and growth of reaction in HE [Lee and Tarver 1980, Cochran and Chan 
1979], 
•  tabulated compaction, 
•  tabulated, 
•  TENSOR pore collapse [Burton et al.  1982]. 
The  ignition  and  growth  EOS  was  adapted  from  KOVEC  [Woodruff  1973];  the  other 
subroutines, programmed by the authors, are based in part on the cited references and 
are nearly 100 percent vectorized.  The forms of the first five equations of state are also 
given in the KOVEC user’s manual and are retained in this manual.  The high explosive 
programmed burn model is described by Giroux [Simo et al.  1988]. 
The  orthotropic  elastic  and  the  rubber  material  subroutines  use  Green-St.    Venant 
strains to compute second Piola-Kirchhoff stresses, which transform to Cauchy stresses.  
The Jaumann stress rate formulation is used with all other materials with the exception 
of one plasticity model which uses the Green-Naghdi rate. 
SPATIAL DISCRETIZATION 
 are presently available.  Currently springs, dampers, beams, membranes, shells, bricks, 
thick shells and seatbelt elements are included. 
The first shell element in DYNA3D was that of Hughes and Liu [Hughes and Liu 1981a, 
1981b, 1981c], implemented as described in [Hallquist et al.  1985, Hallquist and Benson 
1986].  This element [designated as HL] was selected from among a substantial body of 
shell element literature because the element formulation has several desirable qualities:
INTRODUCTION 
Shells
Solids
Beams
Trusses
Springs
Lumped Masses
Damper
  Elements  in  LS-DYNA. 
Figure  1-1. 
  Three-dimensional  plane  stress 
constitutive  subroutines  are  implemented  for  the  shell  elements  which
iteratively  update  the  stress  tensor  such  that  the  stress  component  normal  to
the  shell  midsurface  is  zero.    An  iterative  update  is  necessary  to  accurately 
determine the normal strain component which is necessary to predict thinning.
One  constitutive  evaluation  is  made  for  each  integration  point  through  the
h ll thi k
•  It  is  incrementally  objective  (rigid  body  rotations  do  not  generate  strains), 
allowing for the treatment of finite strains that occur in many practical applica-
tions. 
•  It is compatible with brick elements, because the element is based on a degener-
ated brick element formulation.  This compatibility allows many of the efficient 
and  effective  techniques  developed  for  the  DYNA3D  brick  elements  to  be  used 
with this shell element; 
•  It includes finite transverse shear strains; 
•  A through-the-thickness thinning option  is also 
available. 
All  shells  in  our  current  LS-DYNA  code  must  satisfy  these  desirable  traits  to  at  least 
some extent to be useful in metalforming and crash simulations. 
The  major  disadvantage  of  the  HL  element  turned  out  to  be  cost  related  and,  for  this 
reason, within a year of its implementation we looked at the Belytschko-Tsay [BT] shell 
[Belytschko  and  Tsay  1981,  1983,  1984]  as  a  more  cost  effective,  but  possibly  less 
accurate alternative.  In the BT shell the geometry of the shell is assumed to be perfectly 
flat, the local coordinate system originates at the first node of the connectivity, and the
INTRODUCTION 
co-rotational stress update does not use the costly Jaumann stress rotation.  With these 
and  other  simplifications,  a  very  cost  effective  shell  was  derived  which  today  has 
become  perhaps  the  most  widely  used  shell  elements  in  both  metalforming  and  crash 
applications.  Results generated by the BT shell usually compare favorably with those of 
the more costly HL shell.  Triangular shell elements are implemented, based on work by 
Belytschko  and  co-workers  [Belytschko  and  Marchertas  1974,  Bazeley  et al.    1965, 
Belytschko  et al.    1984],  and  are  frequently  used  since  collapsed  quadrilateral  shell 
elements  tend  to  lock  and  give  very  bad  results.    LS-DYNA  automatically  treats 
collapsed quadrilateral shell elements as C0 triangular elements. 
Since the Belytschko-Tsay element is based on a perfectly flat geometry, warpage is not 
considered.    Although  this  generally  poses  no  major  difficulties  and  provides  for  an 
efficient  element,  incorrect  results  in  the  twisted  beam  problem  and  similar  situations 
are  obtained  where  the  nodal  points  of the elements  used in  the  discretization  are  not 
coplanar.    The  Hughes-Liu  shell  element  considers  non-planar  geometries  and  gives 
good  results  on  the  twisted  beam.    The  effect  of  neglecting  warpage  in  a  typical 
application cannot be predicted beforehand and may lead to less than accurate results, 
but  the  latter  is  only  speculation  and  is  difficult  to  verify  in  practice.    Obviously,  it 
would  be  better  to  use  shells  that  consider  warpage  if  the  added  costs  are  reasonable 
and if this unknown effect is eliminated.  Another shell published by Belytschko, Wong, 
and  Chiang  [Belytschko,  Wong,  and  Chiang  1989,  1992]  proposes  inexpensive 
modifications  to  include  the  warping  stiffness  in  the  Belytschko-Tsay  shell.    An 
improved  transverse  shear  treatment  also  allows  the  element  to  pass  the  Kirchhoff 
patch test.  This element is now available in LS-DYNA.  Also, two fully integrated shell 
elements, based on the Hughes and Liu formulation, are available in LS-DYNA, but are 
rather  expensive.    A  much  faster  fully  integrated  element  which  is  essentially  a  fully 
integrated  version  of  the  Belytschko,  Wong,  and  Chiang  element,  type  16,  is  a  more 
recent addition and is recommended if fully integrated elements are needed due to its 
cost effectiveness. 
Zero energy modes in the shell and solid elements are controlled by either an hourglass 
viscosity or stiffness.  Eight node thick shell elements are implemented and have been 
found to perform well in many applications.  All elements are nearly 100% vectorized.  
All element classes can be included as parts of a rigid body.  The rigid body formulation 
is  documented  in  [Benson  and  Hallquist  1986].    Rigid  body  point  nodes,  as  well  as 
concentrated masses, springs and dashpots can be added to this rigid body. 
Membrane elements can be either defined directly as shell elements with a membrane 
formulation  option  or  as  shell  elements  with  only  one  point  for  through  thickness 
integration.    The  latter  choice  includes  transverse  shear  stiffness  and  may  be 
inappropriate.    For  airbag  material  a  special  fully  integrated  three  and  four  node 
membrane element is available.
INTRODUCTION 
Two different beam types are available: a stress resultant beam and a beam with cross 
section integration at one point along the axis.  The cross section integration allows for a 
more general definition of arbitrarily shaped cross sections taking into account material 
nonlinearities. 
Spring and damper elements can be translational or rotational.  Many behavior options 
can be defined, e.g., arbitrary nonlinear behavior including locking and separation. 
Solid  elements  in  LS-DYNA  may  be  defined  using  from  4  to  8  nodes.    The  standard 
elements  are  based  on  linear  shape  functions  and  use  one  point  integration  and 
hourglass control.  A selective-reduced integrated (called fully integrated) 8 node solid 
element is available for situations when the hourglass control fails.  Also, two additional 
solid  elements,  a  4  noded  tetrahedron  and  an  8  noded  hexahedron,  with  nodal 
rotational degrees of freedom, are implemented based on the idea  of Allman [1984] to 
replace  the  nodal  midside  translational  degrees  of  freedom  of  the  elements  with 
quadratic  shape  functions  by  corresponding  nodal  rotations  at  the  corner  nodes.    The 
latter  elements,  which  do  not  need  hourglass  control,  require  many  numerical 
operations compared to the hourglass controlled elements and should be used at places 
where the hourglass elements fail.  However, it is well known that the elements using 
more  than  one  point  integration  are  more  sensitive  to  large  distortions  than  one  point 
integrated elements. 
The  thick  shell  element  is  a  shell  element  with  only  nodal  translations  for  the  eight 
nodes.  The assumptions of shell theory are included in a non-standard fashion.  It also 
uses  hourglass  control  or  selective-reduced  integration.    This  element  can  be  used  in 
place of any four node shell element.  It is favorably used for shell-brick transitions, as 
no  additional  constraint  conditions  are  necessary.    However,  care  has  to  be  taken  to 
know  in  which  direction  the  shell  assumptions  are  made;  therefore,  the  numbering  of 
the element is important. 
Seatbelt  elements  can  be  separately  defined  to  model  seatbelt  actions  combined  with 
dummy models.  Separate definitions of seatbelts, which are one-dimensional elements, 
with accelerometers, sensors, pretensioners, retractors, and sliprings are possible.  The 
actions of the various seatbelt definitions can also be arbitrarily combined. 
CONTACT-IMPACT INTERFACES 
The  three-dimensional  contact-impact  algorithm  was  originally  an  extension  of  the 
NIKE2D  [Hallquist  1979]  two-dimensional  algorithm.    As  currently  implemented,  one 
surface of the interface is identified as a master surface and the other as a slave.  Each 
surface  is  defined  by  a  set  of  three  or  four node  quadrilateral  segments,  called  master 
and slave segments, on which the nodes of the slave and master surfaces, respectively, 
must slide.  In general, an input for the contact-impact algorithm requires that a list of
INTRODUCTION 
master and slave segments be defined.  For the single surface algorithm only the slave 
surface is defined and each node in the surface is checked each time step to ensure that 
it does not penetrate through the surface.  Internal logic [Hallquist 1977, Hallquist et al.  
1985]  identifies  a  master  segment  for  each  slave  node  and  a  slave  segment  for  each 
master  node  and  updates  this  information  every  time  step  as  the  slave  and  master 
nodes slide along their respective surfaces.  It must be noted that for general automatic 
definitions only parts/materials or three-dimensional boxes have to be given.  Then the 
possible  contacting  outer  surfaces  are  identified  by  the  internal  logic  in  LS-DYNA.  
More than 20 types of interfaces can presently be defined including: 
•sliding only for fluid/structure or gas/structure interfaces 
•tied 
•sliding, impact, friction 
•single surface contact 
•discrete nodes impacting surface 
•discrete nodes tied to surface 
•shell edge tied to shell surface 
•nodes spot welded to surface 
•tiebreak interface 
•one way treatment of sliding, impact, friction 
•box/material limited automatic contact for shells 
•automatic contact for shells (no additional input required) 
•automatic single surface with beams and arbitrary orientations 
•surface to surface eroding contact 
•node to surface eroding contact 
•single surface eroding contact 
•surface to surface symmetric constraint method [Taylor and Flanagan 1989] 
•node to surface constraint method [Taylor and Flanagan 1989] 
•rigid body to rigid body contact with arbitrary force/deflection curve 
•rigid nodes to rigid body contact with arbitrary force/deflection curve 
•edge-to-edge 
•draw beads 
Interface  friction  can  be  used  with  most  interface  types.    The  tied  and  sliding  only 
interface  options  are  similar  to  the  two-dimensional  algorithm  used  in  LS-DYNA2D 
[Hallquist  1976,  1978,  1980].    Unlike  the  general  option,  the  tied  treatments  are  not 
symmetric; therefore, the surface which is more coarsely zoned should be chosen as the 
master  surface.    When  using  the  one-way  slide  surface  with  rigid  materials,  the  rigid 
material should be chosen as the master surface. 
For  geometric  contact  entities,  contact  has  to  be  separately  defined.    It  must  be  noted 
that  for  the  contact  of  a  rigid  body  with  a  flexible  body,  either  the  sliding  interface 
definitions  as  explained  above  or  the  geometric  contact  entity  contact  can  be  used.
INTRODUCTION 
Currently,  the  geometric  contact  entity  definition  is  recommended  for  metalforming 
problems due to high accuracy and computational efficiency.   
INTERFACE DEFINITIONS FOR COMPONENT ANALYSIS 
Interface definitions for component analyses are used to define surfaces, nodal lines, or 
nodal points (*INTERFACE_COMPONENTS) for which the displacement and velocity 
time histories are saved at some user specified frequency (*CONTROL_OUTPUT).  This 
data  may  then  used  to  drive  interfaces  (*INTERFACE_LINKING)  in  subsequent 
analyses.    This  capability  is  especially  useful  for  studying  the  detailed  response  of  a 
small  member  in  a  large  structure.   For  the first  analysis,  the  member  of  interest  need 
only be discretized sufficiently that the displacements and velocities on its boundaries 
are reasonably accurate.  After the first analysis is completed, the member can be finely 
discretized  and  interfaces  defined  to  correspond  with  the  first  analysis.    Finally,  the 
second analysis is performed to obtain highly detailed information in the local region of 
interest. 
When  starting  the  analysis,  specify  a  name  for  the  interface  segment  file  using  the 
Z = parameter on the LS-DYNA command line.  When starting the second analysis, the 
name of the interface segment file (created in the first run) should be specified using the 
L = parameter on the LS-DYNA command line. 
the  above  procedure,  multiple 
levels  of  sub-modeling  are  easily 
Following 
accommodated.    The  interface  file  may  contain  a  multitude  of  interface  definitions  so 
that a single run of a full model can provide enough interface data for many component 
analyses.  The interface feature represents a powerful extension of LS-DYNA’s analysis 
capability. 
PRECISION 
to  machine  precision 
The  explicit  time  integration  algorithms  used  in  LS-DYNA  are  in  general  much  less 
sensitive 
finite  element  solution  methods.  
than  other 
Consequently,  double  precision  is  not  generally  required.    The  benefits  of  this  are 
greatly improved utilization of memory and disk.  When problems have been found we 
have  usually  been  able  to  overcome  them  by  reorganizing  the  algorithm  or  by 
converting  to  double  precision  locally  in  the  subroutine  where  the  problem  occurs.  
Particularly sensitive problems (e.g.  some buckling problems, which can be sensitive to 
small imperfections) may require the fully double precision version, which is available 
on all platforms.  Very large problems requiring more than 2 billion words of memory 
will  also  need  to  be  run  in  double  precision,  due  to  the  array  indexing  limitation  of 
single precision integers.
Getting Started 
GETTING STARTED 
DESCRIPTION OF KEYWORD INPUT 
The keyword input provides a flexible and logically organized database that is simple 
to  understand.    Similar  functions  are  grouped  together  under the  same  keyword.   For 
example,  under  the  keyword  *ELEMENT  are  included  solid,  beam,  shell  elements, 
spring  elements,  discrete  dampers,  seat  belts,  and  lumped  masses.      Many  keywords 
have  options  that  are  identified  as  follows:    “OPTIONS”  and  “{OPTIONS}”.    The 
difference  is  that  “OPTIONS”  requires  that  one  of  the  options  must  be  selected  to 
complete the keyword command.  The option <BLANK> is included when {} are used 
to  further  indicate  that  these  particular  options  are  not  necessary  to  complete  the 
keyword. 
LS-DYNA  User’s  Manual  is  alphabetically  organized  in  logical  sections  of  input  data.  
Each logical section relates to a particular input.  There is a control section for resetting 
LS-DYNA  defaults,  a  material  section  for  defining  constitutive  constants,  an  equation-
of-state  section,  an  element  section  where  element  part  identifiers  and  nodal 
connectivities are defined, a section for defining parts, and so on.  Nearly all model data 
can  be  input  in  block  form.    For  example,  consider  the  following  where  two  nodal 
points with their respective coordinates and shell elements with their part identity and 
nodal connectivity’s are defined: 
$define two nodes 
$ 
*NODE 
10101x y z 
10201x y z 
$    define two shell elements 
$ 
*ELEMENT_SHELL 
10201pidn1n2n3n4 
10301pidn1n2n3n4 
Alternatively, acceptable input could also be of the form: 
$     define one node 
$ 
*NODE 
10101x y z 
$    define one shell element 
$ 
*ELEMENT_SHELL 
10201pidn1n2n3n4 
$ 
$     define one more node 
$ 
*NODE 
10201x y z 
$ define one more shell element 
$ 
*ELEMENT_SHELL 
10301pidn1n2n3n4
Getting Started 
*NODE
*ELEMENT
*PART
NID X Y Z
EID PID N1 N2 N3 N4
PID SID MID EOSID HGID
*SECTION_SHELL
SID ELFORM SHRF NIP PROPT QR ICOMP
*MAT_ELASTIC
MID RO E PR DA DB
*EOS
*HOURGLASS
EOSID
HGID
Figure 2-1.  Organization of  the keyword input. 
A  data  block  begins  with  a  keyword  followed  by  the  data  pertaining  to  the  keyword.  
The next keyword encountered during the reading of the block data defines the end of 
the block and the beginning of a new block.  A keyword must be left justified with the 
“*” contained in column one.  A dollar sign “$” in column one precedes a comment and 
causes the input line to be ignored.  Data blocks are not a requirement for LS-DYNA but 
they  can  be  used  to  group  nodes  and  elements  for  user  convenience.    Multiple  blocks 
can be defined with each keyword if desired as shown above.  It would be possible to 
put  all  nodal  points  definitions  under  one  keyword  *NODE,  or  to  define  one  *NODE 
keyword  prior  to  each  node  definition.    The  entire  LS-DYNA  input  is  order 
independent with the exception of the optional keyword, *END, which defines the end 
of  input  stream.    Without  the  *END  termination  is  assumed  to  occur  when  an  end-of-
file is encountered during the reading. 
Figure  2-1  highlights  how  various  entities  relate  to  each  other  in  LS-DYNA  input.    In 
this  figure  the  data  included  for  the  keyword,  *ELEMENT,  is  the  element  identifier, 
EID,  the  part  identifier,  PID,  and  the  nodal  points  identifiers,  the  NID’s,  defining  the 
element connectivity: N1, N2, N3, and N4.  The nodal point identifiers are defined in the 
*NODE section where each NID should be defined just once.  A part defined with the 
*PART keyword has a unique part identifier, PID, a section identifier, SID, a material or 
constitutive  model  identifier,  MID,  an  equation  of  state  identifier,  EOSID,  and  the 
hourglass  control  identifier,  HGID.    The  *SECTION  keyword  defines  the  section 
identifier,  SID,  where  a  section  has  an  element  formulation  specified,  a  shear  factor, 
SHRF, a numerical integration rule, NIP, among other parameters. 
Constitutive  constants  are  defined  in  the  *MAT  section  where  constitutive  data  is 
defined  for  all  element  types  including  solids,  beams,  shells,  thick  shells,  seat  belts, 
springs,  and  dampers.    Equations  of  state,  which  are  used  only  with  certain  *MAT 
materials  for  solid  elements,  are  defined  in  the  *EOS  section.    Since  many  elements  in 
LS-DYNA  use  uniformly  reduced  numerical  integration,  zero  energy  deformation 
modes  may  develop.    These  modes  are  controlled  numerically  by  either  an  artificial 
stiffness  or  viscosity  which  resists  the  formation  of  these  undesirable  modes.    The 
hourglass control can optionally be user specified using the input in the *HOURGLASS 
section.
Getting Started 
During the keyword input phase where data is read, only limited checking is performed 
on  the  data  since  the  data  must  first  be  counted  for  the  array  allocations  and  then 
reordered.    Considerably  more  checking  is  done  during  the  second  phase  where  the 
input data is printed out.  Since LS-DYNA has retained the option of reading older non-
keyword input files, we print out the data into the output file d3hsp (default name) as 
in  previous  versions  of  LS-DYNA.    An  attempt  is  made  to  complete  the  input  phase 
before  error  terminating  if  errors  are  encountered  in  the  input.    Unfortunately,  this  is 
not  always  possible  and  the  code  may  terminate  with  an  error  message.    The  user 
should always check either output file, d3hsp or messag, for the word “Error”. 
The input data following each keyword can be input in free format.  In the case of free 
format input the data is separated by commas, i.e., 
*NODE 
10101,x ,y ,z 
10201,x ,y ,z 
*ELEMENT_SHELL 
10201,pid,n1,n2,n3,n4 
10301,pid,n1,n2,n3,n4 
When  using  commas,  the  formats  must  not  be  violated.    An  I8  integer  is  limited  to  a 
maximum  positive  value  of  99999999,  and  larger  numbers  having  more  than  eight 
characters  are  unacceptable.    The  format  of  the  input  can  change  from  free  to  fixed 
anywhere in the input file.  The input is case insensitive and keywords can be given in 
either upper or lower case.  The asterisks “*” preceding each keyword must be in column one. 
To  provide  a  better  understanding  behind  the  keyword  philosophy  and  how  the 
options work, a brief review the keywords is given below. 
*AIRBAG 
The  geometric  definition  of  airbags  and  the  thermodynamic  properties  for  the  airbag 
inflator models can be made in this section.  This capability is not necessarily limited to 
the modeling of automotive airbags, but it can also be used for many other applications 
such as tires and pneumatic dampers.  
*ALE 
This  keyword  provides  a  way  of  defining  input  data  pertaining  to  the  Arbitrary-
Lagrangian-Eulerian capability.
This  section  applies  to  various  methods  of  specifying  either  fixed  or  prescribed 
boundary  conditions.    For  compatibility  with  older  versions  of  LS-DYNA  it  is  still 
possible to specify some nodal boundary conditions in the *NODE card section. 
*CASE 
This  keyword  option  provides  a  way  of  running  multiple  load  cases  sequentially.   
Within  each  case,  the  input  parameters,  which  include  loads,  boundary  conditions, 
control  cards,  contact  definitions,  initial  conditions,  etc.,  can  change.    If  desired,  the 
results from a previous case can be used during initialization.  Each case creates unique 
file names for all output results files by appending CIDn to the default file name. 
*COMPONENT 
This  section  contains  analytical  rigid  body dummies  that  can  be  placed  within  vehicle 
and integrated implicitly. 
*CONSTRAINED 
This  section  applies  constraints  within  the  structure  between  structural  parts.    For 
example, nodal rigid bodies, rivets, spot welds, linear constraints, tying a shell edge to a 
shell  edge  with  failure,  merging  rigid  bodies,  adding  extra  nodes  to  rigid  bodies  and 
defining rigid body joints are all options in this section. 
*CONTACT 
This  section  is  divided  in  to  three  main  sections.    The  *CONTACT  section  allows  the 
user  to  define  many  different  contact  types.    These  contact  options  are  primarily  for 
treating  contact  of  deformable  to  deformable  bodies,  single  surface  contact  in 
deformable  bodies,  deformable  body  to  rigid  body  contact,  and  tying  deformable 
structures  with  an  option  to  release  the  tie  based  on  plastic  strain.    The  surface 
definition for contact is made up of segments on the shell or solid element surfaces.  The 
keyword options and the corresponding numbers in previous code versions are: 
STRUCTURED INPUT TYPE ID 
KEYWORD NAME 
1 
p 1 
2 
SLIDING_ONLY 
SLIDING_ONLY_PENALTY 
TIED_SURFACE_TO_SURFACE
3 
a 3 
4 
5 
a 5 
6 
7 
8 
9 
10 
a 10 
13 
a 13 
14 
15 
16 
17 
18 
19 
20 
21 
22 
23 
Getting Started 
SURFACE_TO_SURFACE 
AUTOMATIC_SURFACE_TO_SURFACE 
SINGLE_SURFACE 
NODES_TO_SURFACE 
AUTOMATIC_NODES_TO_SURFACE 
TIED_NODES_TO_SURFACE 
TIED_SHELL_EDGE_TO_SURFACE 
TIEBREAK_NODES_TO_SURFACE 
TIEBREAK_SURFACE_TO_SURFACE 
ONE_WAY_SURFACE_TO_SURFACE 
AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE 
AUTOMATIC_SINGLE_SURFACE  
AIRBAG_SINGLE_SURFACE  
ERODING_SURFACE_TO_SURFACE 
ERODING_SINGLE_SURFACE 
ERODING_NODES_TO_SURFACE 
CONSTRAINT_SURFACE_TO_SURFACE 
CONSTRAINT_NODES_TO_SURFACE 
RIGID_BODY_TWO_WAY_TO_RIGID_BODY 
RIGID_NODES_TO_RIGID_BODY 
RIGID_BODY_ONE_WAY_TO_RIGID_BODY 
SINGLE_EDGE 
DRAWBEAD
Getting Started 
The *CONTACT_ENTITY section treats contact between a rigid surface, usually defined 
as an analytical surface, and a deformable structure.  Applications of this type of contact 
exist  in  the  metal  forming  area  where  the  punch  and  die  surface  geometries  can  be 
input  as  VDA  surfaces  which  are  treated  as  rigid.    Another  application  is  treating 
contact  between  rigid  body  occupant  dummy  hyper-ellipsoids  and  deformable 
structures such as airbags and instrument panels.  This option is particularly valuable in 
coupling  with  the  rigid  body  occupant  modeling  codes  MADYMO  and  CAL3D.    The 
*CONTACT_1D is for modeling rebars in concrete structure. 
*CONTROL 
Options  available  in  the  *CONTROL  section  allow  the  resetting  of  default  global 
parameters  such  as  the  hourglass  type,  the  contact  penalty  scale  factor,  shell  element 
formulation, numerical damping, and termination time. 
*DAMPING 
Defines damping either globally or by part identifier. 
*DATABASE 
This keyword with a combination of options can be used for controlling the output of 
ASCII  databases  and  binary  files  output  by  LS-DYNA.    With  this  keyword  the 
frequency of writing the various databases can be determined. 
*DEFINE 
This  section  allows  the  user  to  define  curves  for  loading,  constitutive  behaviors,  etc.; 
boxes to limit the geometric extent of certain inputs; local coordinate systems; vectors; 
and  orientation vectors  specific  to  spring  and  damper  elements.    Items  defined  in  this 
section  are  referenced  by  their  identifiers  throughout  the  input.    For  example,  a 
coordinate  system  identifier  is  sometimes  used  on  the  *BOUNDARY  cards,  and  load 
curves are used on the *AIRBAG cards.  
*DEFORMABLE_TO_RIGID 
This section allows the user to switch parts that are defined as deformable to rigid at the 
start  of  the  analysis.    This  capability  provides  a  cost  efficient  method  for  simulating 
events such as rollover events.  While the vehicle is rotating the computation cost can be 
reduced significantly by switching deformable parts that are not expected to deform to 
rigid  parts.    Just  before  the  vehicle  comes  in  contact  with  ground,  the  analysis  can  be 
stopped and restarted with the part switched back to deformable.
Define identifiers and connectivities for all elements which include shells, beams, solids, 
thick shells, springs, dampers, seat belts, and concentrated masses in LS-DYNA. 
*EOS 
This  section  reads  the  equations  of  state  parameters.    The  equation  of  state  identifier, 
EOSID, points to the equation of state identifier on the *PART card. 
*HOURGLASS 
Defines  hourglass  and  bulk  viscosity  properties.    The  identifier,  HGID,  on  the 
*HOURGLASS card refers to HGID on *PART card. 
*INCLUDE 
To  make  the  input  file  easy  to  maintain,  this  keyword  allows  the  input  file  to  be  split 
into sub-files.  Each sub-file can again be split into sub-sub-files and so on.  This option 
is beneficial when the input data deck is very large. 
*INITIAL 
Initial velocity and initial momentum for the structure can be specified in this section.  
The initial velocity specification can be made by *INITIAL_VELOCITY_NODE card or 
*INITIAL_VELOCITY  cards.    In  the  case  of  *INITIAL_VELOCITY_NODE  nodal 
identifiers are used to specify the velocity components for the node.  Since all the nodes 
in the system are initialized to zero, only the nodes with non-zero velocities need to be 
specified.    The  *INITIAL_VELOCITY  card  provides  the  capability  of  being  able  to 
specify velocities using the set concept or boxes.  
*INTEGRATION 
In  this  section  the  user  defined  integration  rules  for  beam  and  shell  elements  are 
specified.  IRID refers to integration rule number IRID on *SECTION_BEAM and *SEC-
TION_SHELL  cards  respectively.    Quadrature  rules  in  the  *SECTION_SHELL  and 
*SECTION_BEAM cards need to be specified as a negative number.  The absolute value 
of  the  negative  number  refers  to  user  defined  integration  rule  number.    Positive  rule 
numbers refer to the built in quadrature rules within LS-DYNA.
Interface definitions are used to define surfaces, nodal lines, and nodal points for which 
the displacement and velocity time histories are saved at some user specified frequency.  
This  data  may  then  be  used  in  subsequent  analyses  as  an  interface  ID  in  the  *INTER-
FACE_LINKING_DISCRETE_NODE  as  master  nodes,  in  *INTERFACE_LINKING_-
SEGMENT  as  master  segments  and  in  *INTERFACE_LINKING_EDGE  as  the  master 
edge for a series of nodes. 
This capability is especially useful for studying the detailed response of a small member 
in  a  large  structure.    For  the  first  analysis,  the  member  of  interest  need  only  be 
discretized  sufficiently  that  the  displacements  and  velocities  on  its  boundaries  are 
reasonably  accurate.    After  the  first  analysis  is  completed,  the  member  can  be  finely 
discretized  in  the  region  bounded  by  the  interfaces.    Finally,  the  second  analysis  is 
performed to obtain highly detailed information in the local region of interest. 
When  beginning  the  first  analysis,  specify  a  name  for  the  interface  segment  file  using 
the  Z=parameter  on  the  LS-DYNA  execution  line.    When  starting  the  second  analysis, 
the name of the interface segment file created in the first run should be specified using 
the  L=parameter  on  the  LS-DYNA  command  line.    Following  the  above  procedure, 
multiple  levels  of  sub-modeling  are  easily  accommodated.    The  interface  file  may 
contain  a  multitude  of  interface  definitions  so  that  a  single  run  of  a  full  model  can 
provide  enough  interface  data  for  many  component  analyses.    The  interface  feature 
represents  a  powerful  extension  of  LS-DYNA’s  analysis  capabilities.    A  similar 
capability  using  *INTERFACE_SSI  may  be  used  for  soil-structure  interaction  analysis 
under earthquake excitation. 
*KEYWORD 
Flags LS-DYNA that the input deck is a keyword deck.  To have an effect this must be 
the very first card in the input deck.  Alternatively, by typing “keyword” on the execute 
line,  keyword  input  formats  are  assumed  and the  “*KEYWORD”  is  not  required.    If  a 
number is specified on this card after the word KEYWORD it defines the memory size 
to used in words.  The memory size can also be set on the command line. 
NOTE:  The  memory  specified  on  the  execution  line  over-
rides memory specified on the *keyword card. 
*LOAD 
This section provides various methods of loading the structure with concentrated point 
loads, distributed pressures, body force loads, and a variety of thermal loadings.
This  section  allows  the  definition  of  constitutive  constants  for  all  material  models 
available  in  LS-DYNA  including  springs,  dampers,  and  seat  belts.    The  material 
identifier, MID, points to the MID on the *PART card. 
*NODE 
Define nodal point identifiers and their coordinates. 
*PARAMETER 
This option provides a way of specifying numerical values of parameter names that are 
referenced  throughout  the  input  file.    The  parameter  definitions,  if  used,  should  be 
placed  at  the  beginning  of  the  input  file  following  *KEYWORD.    *PARAMETER_EX-
PRESSION permits general algebraic expressions to be used to set the values. 
*PART 
This keyword serves two purposes. 
1.  Relates part ID to *SECTION, *MATERIAL, *EOS and *HOURGLASS sections. 
2.  Optionally,  in  the  case  of  a  rigid  material,  rigid  body  inertia  properties  and 
initial conditions can be specified.  Deformable material repositioning data can 
also be specified in this section if the reposition option is invoked on the *PART 
card, i.e., *PART_REPOSITION.   
*PERTURBATION 
This keyword provides a way of defining deviations from the designed structure such 
as, buckling imperfections. 
*RAIL 
This  keyword  provides  a  way  of  defining  a  wheel-rail  contact  algorithm  intended  for 
railway applications but can also be used for other purposes.  The wheel nodes (defined 
on *RAIL_TRAIN) represent the contact patch between wheel and rail. 
*RIGIDWALL 
Rigid  wall  definitions  have  been  divided  into  two  separate  sections,  PLANAR  and 
GEOMETRIC.  Planar walls can be either stationary or moving in translational motion
Getting Started 
with  mass  and  initial  velocity.    The  planar  wall  can  be  either  finite  or  infinite.  
Geometric walls can be planar as well as have the geometric shapes such as rectangular 
prism,  cylindrical  prism  and  sphere.    By  default,  these  walls  are  stationary  unless  the 
option MOTION is invoked for either prescribed translational velocity or displacement.  
Unlike the planar walls, the motion of the geometric wall is governed by a load curve.  
Multiple  geometric  walls  can  be  defined  to  model  combinations  of  geometric  shapes 
available.    For  example,  a  wall  defined  with  the  CYLINDER  option  can  be  combined 
with  two  walls  defined  with  the  SPHERICAL  option  to  model  hemispherical  surface 
caps on the two ends of a cylinder.  Contact entities are also analytical surfaces but have 
the  significant  advantage  that  the  motion  can  be  influenced  by  the  contact  to  other 
bodies, or prescribed with six full degrees-of-freedom. 
*SECTION 
In  this  section,  the  element  formulation,  integration  rule,  nodal  thicknesses,  and  cross 
sectional properties are defined.  All section identifiers (SECID’s) defined in this section 
must  be  unique,  i.e.,  if  a  number  is  used  as  a  section  ID  for  a  beam  element  then  this 
number cannot be used again as a section ID for a solid element. 
*SENSOR 
This  keyword  provides  a  convenient  way  of  activating  and  deactivating  boundary 
conditions,  airbags,  discrete  elements, 
joints,  contact,  rigid  walls,  single  point 
constraints, and constrained nodes.   The sensor capability is new in the second release 
of  version  971  and  will  evolve  in  later  releases  to  encompass  many  more  LS-DYNA 
capabilities and replace some of the existing capabilities such as the airbag sensor logic. 
*SET 
A concept of grouping nodes, elements, materials, etc., in sets is employed throughout 
the LS-DYNA input deck.  Sets of data entities can be used for output.  So-called slave 
nodes  used  in  contact  definitions,  slaves  segment  sets,  master  segment  sets,  pressure 
segment sets and so on can also be defined.  The keyword, *SET, can be defined in two 
ways: 
1.  Option  LIST  requires  a  list  of  entities,  eight  entities  per  card,  and  define  as 
many cards as needed to define all the entities. 
2.  Option  COLUMN,  where  applicable,  requires  an  input  of  one  entity  per  line 
along  with  up  to  four  attribute  values  which  are  used  by  other  keywords  to 
specify, for example, the failure criterion input that is needed for *CONTACT_-
CONSTRAINT_NODES_TO_SURFACE.
This  keyword  provides  an  alternative  way  of  stopping  the  calculation  before  the 
termination time is reached.  The termination time is specified on the *CONTROL_TER-
MINATION  input  and  will  terminate  the  calculation  whether  or  not  the  options 
available in this section are active. 
*TITLE 
In this section a title for the analysis is defined. 
*USER_INTERFACE 
This  section  provides  a  method  to  provide user  control  of  some  aspects  of  the  contact 
algorithms including friction coefficients via user defined subroutines.  
RESTART 
This  section  of  the  input  is  intended  to  allow  the  user  to  restart  the  simulation  by 
providing  a  restart  file  and  optionally  a  restart  input  defining  changes  to  the  model 
such  as  deleting  contacts,  materials,  elements,  switching  materials  from  rigid  to 
deformable, deformable to rigid, etc. 
*RIGID_DEFORMABLE 
This section switches rigid parts back to deformable in a restart to continue the event of 
a part impacting the ground which may have been modeled with a rigid wall. 
*STRESS_INITIALIZATION 
This is an option available for restart runs.  In some cases there may be a need for the 
user to add contacts, elements, etc., which are not available options for standard restart 
runs.    A  full  input  containing  the  additions  is  needed  if  this  option  is  invoked  upon 
restart.
Getting Started 
SUMMARY OF COMMONLY USED OPTIONS 
The following table gives a list of the commonly used keywords related by topic. 
Topic 
Component 
Keywords 
Nodes 
Elements 
Geometry 
Discrete Elements 
Part 
Material 
Materials 
Sections 
Discrete sections 
*NODE 
*ELEMENT_BEAM 
*ELEMENT_SHELL 
*ELEMENT_SOLID 
*ELEMENT_TSHELL 
*ELEMENT_DISCRETE 
*ELEMENT_SEATBELT 
*ELEMENT_MASS 
PART cards glues the model together: 
⎧*MAT
{{
*SECTION
{{⎨
*EOS
⎩
*HOURGLASS
*PART →
*MAT 
*SECTION_BEAM 
*SECTION_SHELL 
*SECTION_SOLID 
*SECTION_TSHELL 
*SECTION_DISCRETE 
*SECTION_SEATBELT 
Equation of state 
*EOS 
Hourglass 
Contacts & 
Rigid walls 
Defaults for contacts 
Definition of contacts 
Definition of rigid walls 
*CONTROL_HOURGLASS 
*HOURGLASS 
*CONTROL_CONTACT 
*CONTACT_OPTION 
*RIGIDWALL_OPTION
Topic 
Component 
Keywords 
Getting Started 
Boundary 
Conditions & 
Loadings 
Constraints 
and spot 
welds 
Output 
Control 
Restraints 
Gravity (body) load 
Point load 
Pressure load 
Thermal load 
Load curves 
Constrained nodes 
Welds 
Rivet 
*NODE 
*BOUNDARY_SPC_OPTION 
*LOAD_BODY_OPTION 
*LOAD_NODE_OPTION 
*LOAD_SEGMENT_OPTION 
*LOAD_SHELL_OPTION 
*LOAD_THERMAL_OPTION 
*DEFINE_CURVE 
*CONSTRAINED_NODE_SET 
*CONSTRAINED_GENERALIZED_WELD 
*CONSTRAINED_SPOT_WELD 
*CONSTRAINED_RIVET 
Items in time history blocks 
*DATABASE_HISTORY_OPTION 
Default 
ASCII time history files 
*CONTROL_OUTPUT 
*DATABASE_OPTION 
Binary  plot/time  history/restart 
files 
*DATABASE_BINARY_OPTION 
Nodal reaction output 
*DATABASE_NODAL_FORCE_GROUP 
Termination 
Termination time 
Termination cycle 
CPU termination 
Degree of freedom 
*CONTROL_TERMINATION 
*CONTROL_TERMINATION 
*CONTROL_CPU 
*TERMINATION_NODE 
Table 2.1.  Keywords for the most commonly used options. 
EXECUTION SYNTAX 
The  execution  line  for  LS-DYNA,  sometimes  referred  to  as  the  command  line,  is  as 
follows:
Getting Started 
LS-DYNA  I=inf  O=otf  G=ptf  D3PART=d3part  D=dpf  F=thf  T=tpf  A=rrd 
M=sif  S=iff  H=iff  Z=isf1  L=isf2  B=rlf  W=root  E=efl  X=scl  C=cpu  K=kill 
V=vda  Y=c3d  BEM=bof  {KEYWORD}  {THERMAL}  {COUPLE}  {INIT} 
{CASE}  {PGPKEY}  MEMORY=nwds  MODULE=dll  NCPU=ncpu  PA-
RA=para 
JOBID=jobid 
D3PROP=d3prop GMINP=gminp GMOUT=gmout MCHECK=y 
NCYCLE=ncycle 
ENDTIME=time 
where, 
inf  = 
input file (user specified) 
otf   =   high speed printer file (default = d3hsp) 
ptf   =   binary plot file for postprocessing (default = d3plot)  
  d3part   =   binary  plot  file  for  subset  of  parts;  see  *DATABASE_BINARY_D3PART 
(default = d3part) 
dpf  =  dump file to write for purposes of restarting (default = d3dump).  This file 
is  written  at  the  end  of  every  run  and  during  the  run  as  requested  by 
*DATABASE_BINARY_D3DUMP.    To  stop  the  generation  of  this  dump 
file, specify “d=nodump” (case insensitive). 
thf  =  binary plot file for time histories of selected data (default = d3thdt) 
tpf  =  optional temperature file 
rrd   =   running restart dump file (default = runrsf) 
sif  =  stress initialization file (user specified) 
iff  = 
interface  force  file  (user  specified).    See  *DATBASE_BINARY_INTFOR 
and *DATABASE_BINARY_FSIFOR. 
isf1   =   interface segment save file to be created (default = infmak) 
isf2  =  existing interface segment save file to be used (user specified) 
rlf   =   binary plot file for dynamic relaxation (default = d3drfl) 
efl   =  echo  file  containing  optional  input  echo  with  or  without  node/element 
data 
root  =  root file name for general print option 
scl  =  scale factor for binary file sizes (default  =70) 
cpu  =  cumulative  cpu  time  limit  in  seconds  for  the  entire  simulation,  including 
all restarts, if cpu is positive.  If cpu is negative, the absolute value of cpu 
is the cpu time limit in seconds for the first run and for each  subsequent 
restart run. 
kill   =   if  LS-DYNA  encounters  this  file  name  it  will  terminate  with  a restart  file 
(default = d3kil)
Getting Started 
vda  =  VDA/IGES database for geometrical surfaces 
c3d  =  CAL3D input file 
bof  =  *FREQUENCY_DOMAIN_ACOUSTIC_BEM output file 
  nwds  =  Number  of  words  to  be  allocated.    On  engineering  workstations  a  word 
isusually  32bits.    This  number  overwrites  the  memory  size  specified  on 
the *KEYWORD card at the beginning of the input deck. 
dll  =  The dynamic library for user subroutines.  Only one dynamic library can 
be  loaded  via  “module=dll”.    See  *MODULE_LOAD  command  for  load-
ing multiple dynamic libraries. 
  ncpu  =  Overrides  NCPU  and  CONST  defined  in  *CONTROL_PARALLEL.    A 
positive value sets CONST = 2 and a negative values sets CONST = 1.  See 
the  *CONTROL_PARALLEL  command  for  an  explanation  of  these  pa-
rameters.  The *KEYWORD command provides an alternative way to set 
the number of CPUs. 
para  =  Overrides PARA defined in *CONTROL_PARALLEL. 
time  =  Overrides ENDTIM defined in *CONTROL_TERMINATION. 
  ncycle  =  Overrides ENDCYC defined in *CONTROL_TERMINATION. 
jobid  =  Character  string  which  acts  as  a  prefix  for  all  output  files.    Maximum 
length is 72 characters.  Do not include the following characters:  ) (* / ? \. 
  d3prop  =  See *DATABASE_BINARY_D3PROP input parameter IFILE for options. 
  gminp   =   Input  file  for  reading  recorded  motions  in  *INTERFACE_SSI  (default = 
gmbin). 
  gmout   =   Output  file  for  writing  recorded  motions  in  *INTERFACE_SSI_AUX 
(default = gmbin). 
In  order  to  avoid  undesirable  or  confusing  results,  each  LS-DYNA  run  should  be 
performed  in  a  separate  directory,  unless  using  the  command  line  parameter  “jobid” 
described  above.    If  rerunning  a  job  in  the  same  directory,  old  files  should  first  be 
removed  or  renamed  to  avoid  confusion  since  the  possibility  exists  that  the  binary 
database may contain results from both the old and new run. 
By including “keyword” anywhere on the execute line or instead if *KEYWORD is the 
first  card  in  the  input  file,  the  keyword  formats  are  expected;  otherwise,  the  older 
structured input file will be expected. 
To run a coupled thermal analysis the command “couple” must be in the execute line.  
A thermal only analysis may be run by including the word “thermal” in the execution 
line.
Getting Started 
The execution line option “pgpkey” will output the current public PGP key used by LS-
DYNA for encryption of input.  The public key and some instructions on how to use the 
key are written  to the screen as well as a file named “lstc_pgpkey.asc”. 
The  “init”  (or  sw1.  can  be  used  instead)  command  on  the  execution  line  causes  the 
calculation  to  run  just  one  cycle  followed  by  termination  with  a  full  restart  file.    No 
editing  of  the  input  deck  is  required.    The  calculation  can  then  be  restarted  with  or 
without any additional input.  Sometimes this option can be used to reduce the memory 
on  restart  if  the  required  memory  is  given  on  the  execution  line  and  is  specified  too 
large in the beginning when the amount of  required memory is unknown.  Generally, 
this option would be used at the beginning of a new calculation. 
If  the  word  “case”  appears  on  the  command  line,  then  *CASE  statements  will  be 
handled  by  the  built  in  driver  routines.    Otherwise  they  should  be  processed  by  the 
external  “lscasedriver”  program,  and  if  any  *CASE  statements  are  encountered  it  will 
cause an error. 
If “mcheck=y” is given on the command line, the program switches to “model check” 
mode.  In this mode the program will run only 10 cycles – just enough to verify that the 
model  will  start.    For  implicit  problems,  all  initialization  is  performed,  but  execution 
halts  before  the  first  cycle.    If  the  network  license  is  being  used,  the  program  will 
attempt to check out a license under the program name “LS-DYNAMC” so as not to use 
up  one  of  the  normal  DYNA  licenses.    If  this  fails,  a  normal  execution  license  will  be 
used. 
If  the  word  “memory”  is  found  anywhere  on  the  execution  line  and  if  it  is  not  set  via 
“memory=nwds”  LS-DYNA  will  give  the  default  size  of  memory,  request,  and  then 
read  in  the  desired  memory  size.    This  option  is  necessary  if  the  default  value  is 
insufficient memory and termination occurs as a result.  Occasionally, the default value 
is too large for execution and this option can be used to lower the default size.  Memory 
can also be specified on the *KEYWORD card. 
SENSE SWITCH CONTROLS 
The status of an in-progress LS-DYNA simulation can be determined by using the sense 
switch.    On  UNIX  versions,  this  is  accomplished  by  first  typing  a  “^C”  (Control-C).  
This  sends  an  interrupt  to  LS-DYNA  which  is  trapped  and  the  user  is  prompted  to 
input the sense switch code.  LS-DYNA has nine terminal sense switch controls that are 
tabulated below: 
Response 
A restart file is written and LS-DYNA terminates. 
Type 
SW1.
Getting Started 
Type 
SW2. 
SW3. 
SW4. 
SW5. 
SW7. 
SW8. 
SW9. 
SWA. 
lprint 
Response 
LS-DYNA responds with time and cycle numbers. 
A restart file is written and LS-DYNA continues. 
A plot state is written and LS-DYNA continues. 
Enter interactive graphics phase and real time visualization. 
Turn off real time visualization. 
Interactive  2D  rezoner 
visualization. 
for  solid  elements  and  real 
time 
Turn off real time visualization (for option SW8). 
Flush ASCII file buffers. 
Enable/Disable  printing  of  equation  solver  memory,  cpu 
requirements. 
nlprint 
Enable/Disable  printing  of  nonlinear  equilibrium 
information. 
iteration 
iter 
conv 
stop 
Enable/Disable  output  of  binary  plot  database  "d3iter"  showing 
mesh  after  each  equilibrium  iteration.    Useful  for  debugging 
convergence problems. 
Temporarily override nonlinear convergence tolerances. 
Halt execution immediately, closing open files. 
On UNIX/LINUX and Windows systems the sense switches can still be used if the job is 
running  in  the  background  or  in  batch  mode.    To  interrupt  LS-DYNA  simply  create  a 
file called d3kil containing the desired sense switch, e.g., "sw1." LS-DYNA periodically 
looks  for  this  file  and  if  found,  the  sense  switch  contained  therein  is  invoked  and  the 
d3kil file is deleted.  A null d3kil file is equivalent to a "sw1." 
When LS-DYNA terminates, all scratch files are destroyed: the restart file, plot files, and 
high-speed  printer  files  remain  on  disk.    Of  these,  only  the  restart  file  is  needed  to 
continue the interrupted analysis.
Getting Started 
PROCEDURE FOR LS-DYNA/MPP 
As described above the serial/SMP code supports the use of the SIGINT signal (usually 
Ctrl-C) to interrupt the execution and prompt the user for a "sense switch."   The MPP 
code  also  supports  this  capability.    However,  on  many  systems  a  shell  script  or  front 
end program (generally "mpirun") is required to start MPI applications.  Pressing Ctrl-C 
on  some  systems  will  kill  this  process,  and  thus  kill  the  running  MPP-DYNA 
executable.    On  UNIX/LINUX  systems,  as  workaround,  when  the  MPP  code  begins 
execution  it  creates  a  file  named,  “bg_switch”,  in  the  current  working  directory.    This 
file contains the following single line: 
rsh <machine name> kill -INT <PID> 
where <machine name> is the hostname of the machine on which the root MPP-DYNA 
process  is  running,  and  <PID>  is  its  process  id.    (on  HP  systems,  "rsh"  is  replaced  by 
"remsh").    Thus,  simply  executing  this  file  will  send  the  appropriate  signal.    For 
Windows, usually the D3KIL file is used to interrupt the execution. 
For more information about running the LS-DYNA/MPP Version see Appendix O.
Input
Stress Initialization
Restart
Interface Segment
VDA Geometry
I=
=
R=
L=
V =
=
Thermal File
=
CAL3D Input
Getting Started 
Files: Input and Output
Restart Files
D=d3dump
A=runrsf
Z=
Restart Dump
Running Dump
Interface Segment
LS-DYNA
Binary Output
G=d3plot
F=d3dht
S=
B=d3drfl
"d3plot"
Time History
Interface Force
Dynamic Relaxation
O=d3hsp
E=
Text Output
Printer File
"messag"
Input Echo
Others...
Figure 2-2.  Files Input and Output. 
1.  Uniqueness.  File names must be unique. 
FILES 
2. 
Interface forces.  The interface force file is created only if it is specified on the 
execution line “S=iff”. 
3.  File size limits.  For very large models, the default size limits for binary output 
files may not be large enough for a single file to hold even a single plot state, in
Getting Started 
which  case  the  file  size  limit  may  be  increased  by  specifying  “X=scl"  on  the 
execution  line.      The  default  file  size  limit  (X=70)  is  70  times  one-million  octal 
words or 18.35 Mwords.  That translates into 73.4 Mbytes (for 32-bit output) or 
146.8 Mbytes (for 64-bit output).   
4.  CPU limits.  Using “C=cpu” defines the maximum CPU usage allowed.  When 
the  CPU  usage  limit  is  exceeded  LS-DYNA  will  terminate  with  a  restart  file.  
During  a  restart,  cpu  should  be  set  to  the  total  CPU  used  up  to  the  current 
restart plus whatever amount of additional time is wanted. 
5.  File  usage  in  restart.    When  restarting  from  a  dump  file,  the  execution  line 
becomes 
LS-DYNA  I=inf  O=otf  G=ptf  D=dpf  R=rtf  F=thf  T=tpf  A=rrd  S=iff  Z=isf1 
L=isf2  B=rlf  W=root  E=efl  X=scl  C=cpu  K=kill  Q=option  KEYWORD 
MEMORY=nwds 
where, 
rtf=[name of dump file written by LS-DYNA] 
The root names of the dump files written by LS-DYNA = are controlled by dpf 
(default = d3dump) and rrd (default = runrsf).  A two-digit number follows the 
root name, e.g., d3dump01, d3dump02, etc., to distinguish one dump file from 
another.  Typically, each dump file corresponds to a different simulation time. 
The adaptive dump files contain all information required to successfully restart 
so that no other files are needed except when CAD surface data is used.  When 
restarting a problem that uses VDA/IGES surface data, the vda input file must 
be specified, e.g.: 
LS-DYNA R=d3dump01 V=vda 
If the data from the last run is to be remapped onto a new mesh, then specify: 
“Q=remap”.  The remap file is the dump file from which the remapping data is 
taken.  The remap option is available in SMP for brick elements only, MPP does 
not support this option currently. 
No stress initialization is possible at restart.  Also the VDA files and the CAL3D files 
must not be changed. 
6.  Default  file  names.    File  name  dropouts  are  permitted;  for  example,  the 
following execution lines are acceptable: 
LS-DYNA I=inf 
and
Getting Started 
LS-DYNA R=rtf 
7. 
Interface  segments.    For  an  analysis  using  interface  segments,  the  execution 
line in the first analysis is given by: 
and in the second by: 
LS-DYNA I=inf Z=isf1 
LS-DYNA I=inf L=isf1 
8.  Batch  execution.    In  some  installations  (e.g.,  GM)  calculations  are  controlled 
by  a  file  called  “names”  on  unit  88.    The  names  files  consists  of  two  lines  in 
which the second line  is blank.   The first line of names contains the execution 
line, for instance: 
For a restart the execution line becomes: 
I=inf 
I=inf R=rtf 
RESTART ANALYSIS 
The LS-DYNA restart capability allows analyses to be broken down into stages.  After 
the completion of each stage in the calculation a “restart dump” is written that contains 
all  information  necessary  to  continue  the  analysis.    The  size  of  this  “dump”  file  is 
roughly  the  same  size  as  the  memory  required  for  the  calculation.    Results  can  be 
checked at each stage by post-processing the output databases in the normal way, so the 
chance of wasting computer time on incorrect analyses is reduced. 
The  restart  capability  is  frequently  used  to  modify  models  by  deleting  excessively 
distorted elements, materials that are no longer important, and contact surfaces that are 
no  longer  needed.    Output  frequencies  of  the  various  databases  can  also  be  altered.  
Often,  these  simple  modifications  permit  a  calculation  that  might  otherwise  not  to 
continue  on  to  a  successful  completion.    Restarting  can  also  help  to  diagnose  why  a 
model  is  giving  problems.    By  restarting  from  a  dump  that  is  written  before  the 
occurrence of a numerical problem and obtaining output at more frequent intervals, it is 
often  possible  to  identify  where  the  first  symptoms  appear  and  what  aspect  of  the 
model is causing them. 
The format of the restart input file is described in this manual.  If, for example, the user 
wishes  to  restart  the  analysis  from  dump  state  nn,  contained  in  file  D3DUMPnn,  then 
the following procedure is followed:
Getting Started 
1.  Create the restart input deck, if required, as described in the Restart Section of 
this manual.  Call this file restartinput. 
2.  Start dyna from the command line by invoking: 
LS-DYNA I=restartinput R=D3DUMPnn 
3. 
If no alterations to the model are made, then the execution line: 
LS-DYNA R=D3DUMPnn 
will  suffice.    Of  course,  the  other  output  files  should  be  assigned  names  from 
the command line if the defaults have been changed in the original run. 
The  full  deck  restart  option  allows  the  user  to  begin  a  new  analysis,  with  deformed 
shapes  and  stresses  carried  forward  from  a  previous  analysis  for  selected  materials.  
The new analysis can be different from the original, e.g., more contact surfaces, different 
geometry  (of  parts  which  are  not  carried  forward),  etc.    Examples  of  applications 
include: 
•  Crash analysis continued with extra contact surfaces; 
•  Sheet  metalforming  continued  with  different  tools  for  modeling  a  multi-stage 
forming process. 
A typical restart file scenario: 
Dyna  is  run  using  an  input  file  named  “job1.inf”,  and  a  restart  dump  named 
“d3dump01”  is  created.    A  new  input  file,  “job2.inf”,  is  generated  and  submitted  as  a 
restart  with,  “R=d3dump01”,  as  the  dump  file.    The  input  file  job2.inf  contains  the 
entire model in its original undeformed state but with more contact surfaces, new output 
databases, and so on. 
Since this is a restart job, information must be given to tell LS-DYNA which parts of the 
model  should  be  initialized  in  the  full  deck  restart.    When  the  calculation  begins  the 
restart database contained in the file d3dump01 is read, and a new database is created 
to initialize the model in the input file, job2.inf.  The data in file job2.inf is read and the 
LS-DYNA proceeds through the entire input deck and initialization.  At the end of the 
initialization  process,  all  the  parts  selected  are  initialized  from  the  data  saved  from 
d3dump01.  This means that the deformed  position and velocities of the nodes on the 
elements of each part, and the stresses and strains in the elements (and, if the material 
of the part is rigid, the rigid body properties) will be assigned. 
It is assumed during this process that any initialized part has the same elements, in the 
same order, with the same topology, in job1 and job2.  If this is not the case, the parts 
cannot be initialized.  However, the parts may have different identifying numbers.
Getting Started 
For  discrete elements  and  seat  belts,  the  choice  is  all  or  nothing.   All  discrete  and  belt 
elements,  retractors,  sliprings,  pretensioners  and  sensors  must  exist  in  both  files  and 
will be initialized. 
Materials  which  are  not  initialized  will  have  no  initial  deformations  or  stresses.  
However, if initialized and non-initialized materials have nodes in common, the nodes 
will be moved by the initialized material causing a sudden strain in the non-initialized 
material.  This effect can give rise to sudden spikes in loading. 
Points to note are: 
•  Time and output intervals are continuous with job1, i.e., the time is not reset to 
zero. 
•  Don’t try to use the restart part of the input to change anything since this will be 
overwritten by the new input file. 
•  Usually, the complete input file part of job2.inf will be copied from job1.inf, with 
the  required  alterations.    We  again  mention  that  there  is  no  need  to  update  the 
nodal  coordinates  since  the  deformed  shapes  of  the  initialized  materials  will  be 
carried forward from job1. 
•  Completely new databases will be generated with the time offset. 
VDA/IGES DATABASES 
VDA  surfaces  are  surfaces  of  geometric  entities  which  are  given  in  the  form  of 
polynomials.  The format of these surfaces is as defined by the German automobile and 
supplier industry in the VDA guidelines, [VDA 1987]. 
The  advantage  of  using  VDA  surfaces  is  twofold.    First,  the  problem  of  meshing  the 
surface  of  the  geometric  entities  is  avoided  and,  second,  smooth  surfaces  can  be 
achieved  which  are  very  important  in  metalforming.    With  smooth  surfaces,  artificial 
friction introduced by standard faceted meshes with corners and edges can be avoided.  
This is a big advantage in springback calculations. 
A  very  simple  and  general  handling  of  VDA  surfaces  is  possible  allowing  arbitrary 
motion and generation of surfaces.  For a detailed description, see Appendix L.
Getting Started 
ASCII
Databases
Plot Files:
d3plot
d3thdt
Geometry:
i=
iges:
v=
vda:
Project: p=
Keyword: k=
Command: c=
Database: d=
LS-PrePost
Nastran: n=
Graphic Output
Fringe Plots
Time History
Animations
Keyword
Files
Project File
(*.proj)
Command File:
cfile
Database File:
post.db
Figure 2-3.  File Organization 
LS-PrePost® 
LS-DYNA is designed to operate with a variety of commercial pre- and post-processing 
packages.  Currently, direct support is available from TRUEGRID, PATRAN, eta/VPG, 
HYPERMESH,  EASi-CRASH  DYNA  and  FEMAP.    Several  third-party  translation 
programs are available for PATRAN and IDEAS. 
Alternately,  the  pre-  and  post-processor  LS-PrePost  is  available  from  LSTC  and  is 
specialized  for  LS-DYNA.    LS-PrePost  is  an  advanced  pre-  and  post-processor  that  is 
delivered  free  with  LS-DYNA.    The  user  interface  is  designed  to  be  both  efficient  and 
intuitive.  LS-PrePost runs on Windows, Linux, and Unix, utilizing OpenGL graphics to 
achieve fast model rendering and XY plotting. 
Some of the capabilities available in LS-PrePost are: 
•  Complete support for all LS-DYNA keyword data. 
•  Importing  and  combining  multiple  models  from  many  sources  (LS-DYNA 
keyword, IDEAS neutral file, NASTRAN bulk data, STL ASCII, and STL binary 
formats). 
•  Improved renumbering of model entities. 
•  Model Manipulation:  Translate, Rotate, Scale, Project, Offset, Reflect
Getting Started 
•  LS-DYNA  Entity  Creation:    Coordinate  Systems,  Sets,  Parts,  Masses,  CNRBs, 
Boxes,  Spot  welds,  SPCs,  Rigidwalls,  Rivets,  Initial  Velocity,  Accelerometers, 
Cross Sections, etc. 
•  Mesh  Generation:    2Dmesh  Sketchboard,  nLine  Meshing,  Line  sweep  into  shell, 
Shell  sweep  into  solid,  Tet-Meshing,  Automatic  surface  meshing  of  IGES  and 
VDA data, Meshing of simple geometric objects (Plate, Sphere, Cylinder) 
•  Special Applications:  Airbag folding, Dummy positioning, Seatbelt fitting, Initial 
penetration check, Spot weld generation using MAT_100 
•  Complete  support  of  LS-DYNA  results  data  file:    d3plot  file,  d3thdt  file,  All 
ASCII time history data file, Interface force file 
LS-PrePost  processes  output  from  LS-DYNA.    LS-PrePost  reads  the  binary  plot-files 
generated  by  LS-DYNA  and  plots  contours,  fringes,  time  histories,  and  deformed 
shapes.  Color contours and fringes of a large number of quantities may be interactively 
plotted  on  meshes  consisting  of  plate,  shell,  and  solid  type  elements.    LS-PrePost  can 
compute a variety of strain measures, reaction forces along constrained boundaries. 
LS-DYNA  generates  three  binary  databases.    One  contains  information  for  complete 
states  at  infrequent  intervals;  50  to  100  states  of  this  sort  is  typical  in  a  LS-DYNA 
calculation.    The  second  contains  information  for  a  subset  of  nodes  and  elements  at 
frequent intervals; 1000 to 10,000 states is typical.  The third contains interface data for 
contact surfaces.
Getting Started 
 24
 20
 16
 12
 8
 4
 0
20.01
8.84
1.07
1.25
1.28
1.49
2.45
2.80
BT
BTW BL
BWC CHL HL
FBT CFHL FHL
Element type
Figure    2-4.    Relative  cost  of  the  four  noded  shells  available  in  LS-DYNA
where BT is the Belytschko-Tsay shell, BTW is the Belytschko-Tsay shell with
the  warping  stiffness  taken  from  the  Belytschko-Wong-Chiang,  BWC,  shell.
The BL shell  is  the  Belytschko-Leviathan shell.  CHL denotes  the Hughes-Liu
shell, HL, with one point quadrature and a co-rotational formulation.  FBT is a
Belytschko-Tsay  like  shell  with  full  integration,  FHL  is  the  fully  integrated
Hughes-Liu shell, and the CFHL shell is its co-rotational version. 
EXECUTION SPEEDS 
The relative execution speeds for various elements in LS-DYNA are tabulated below: 
Element Type 
Relative Cost 
8  node  solid  with  1  point  integration  and  default 
hourglass control 
as above but with Flanagan-Belytschko hourglass control 
constant  stress  and  Flanagan-Belytschko  hourglass 
control, i.e., the Flanagan-Belytschko element 
4  node  Belytschko-Tsay  shell  with  four  thickness 
integration points 
4 node Belytschko-Tsay shell with resultant plasticity 
4 
5 
7 
4
Element Type 
Relative Cost 
Getting Started 
BCIZ  triangular  shell  with  four  thickness  integration 
points 
Co triangular shell with four thickness integration points 
2 node Hughes-Liu beam with four integration points 
2 node Belytschko-Schwer beam 
2 node simple truss elements 
7 
4 
9 
2 
1 
8 node solid-shell with four thickness integration points 
11 
These  relative  timings  are  very  approximate.    Each  interface  node  of  the  sliding 
interfaces is roughly equivalent to one-half zone cycle in cost.  Figure 2-4.  illustrates the 
relative cost of the various shell formulations in LS-DYNA.  
UNITS 
The units in LS-DYNA must be consistent.  One way of testing whether a set of units is 
consistent is to check that: 
[force unit] =   [mass unit] × [acceleration unit] 
and that 
[acceleration unit] =
[length unit]
[time unit]2 . 
Examples  of  sets  of  consistent  units  are  tabulated  below.    For  a  more  comprehensive 
table, see http://ftp.lstc.com/anonymous/outgoing/support/FAQ/consistent_units . 
(a) 
(b) 
(c) 
Length unit 
Time unit 
Mass unit 
Force unit 
Young’s Modulus of Steel 
Density of Steel 
Yield stress of Mild Steel 
Acceleration due to gravity 
Velocity equivalent to 30 mph 
meter 
second 
kilogram 
Newton 
210.0E+09 
7.85E+03 
200.0E+06 
9.81 
13.4 
millimeter 
second 
tonne 
Newton 
210.0E+03 
7.85E–09 
200.0 
9.81E+03 
13.4E+03 
millimeter 
millisecond 
kilogram 
kiloNewton 
210.0 
7.85E–06 
0.200 
9.81E-03 
13.4
Getting Started 
GENERAL CARD FORMAT 
The  following  sections  specify,  for  each  keyword  command,  the  cards  that  must  be 
defined  and  those  cards  that  are  optional.    Each  card  is  described  in  its  fixed  format 
form and is shown as a number of fields in an 80 character string.  With the exception of 
“long format input” as described later in this section, most cards are 8 fields with a field 
length  of  10  characters.    A  sample  card  is  shown  below.    The  card  format  is  clearly 
stated when it is different than 8  fields of 10 characters.   
As  an  alternative  to  fixed  format,  a  card  may  be  in  free  format  with  the  values  of  the 
variables  separated  by  commas.    When  using  comma-delimited  values  on  a  card,  the 
number of characters used to specify a value must not exceed the field length for fixed 
format.    For  example,  an  I8  number  is  limited  to  a  value  of  99999999  and  a  larger 
number  with  more  than  8  characters  is  unacceptable.    A  further  restriction  is  that 
characters  beyond  column  80  of  each  line  are  ignored  by  the  code.    Fixed  format  and 
free,  comma-delimited  format  can  be  mixed  throughout  the  deck  and  even  within 
different cards of a single command but not within a card. 
The  limits  on  number  of  characters  per  variable  and  number  of  characters  per  line  as 
stated  above  are  raised  in  the  case  of  long  format  input.    See  the  description  of  long 
format input below. 
Example Card. 
 Card [N] 
1 
2 
Variable 
NSID 
PSID 
Type 
I 
I 
3 
A1 
F 
4 
A2 
F 
Default 
none 
none 
1.0 
1.0 
Remarks 
1 
2 
5 
A3 
F 
0 
6 
KAT 
I 
1 
3 
7 
8 
In  the  example  shown  above,  the  row  labeled  “Type”  gives  the  variable  type  and  is 
either  F,  for  floating  point  or  I,  for  an  integer.    The  row  labeled  “Default”  reveals  the 
default value set for a variable if zero is specified, the field is left  blank, or the card is 
not  defined.    The  “Remarks”  row  refers  to  enumerated  remarks  at  the  end  of  the 
section.
Getting Started 
Optional Cards: 
Each  keyword  card  (line  beginning  with  “*”)  is  followed  by  a  set  of  data  cards.    Data 
cards are either, 
1.  Required Cards.  Unless otherwise indicated, cards are required. 
2.  Conditional Cards.  Conditional cards are required provided some condition is 
satisfied.  The following is a typical conditional card: 
ID Card.  Additional card for the ID keyword option.  
ID 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ABID 
Type 
I 
HEADING 
A70 
3.  Optional  Cards.    An  optional  card  is  one  that  may  be  replaced  by  the  next 
keyword card.  The fields in the omitted optional data cards are assigned their 
default values. 
Example.    Suppose  the  data  set  for  *KEYWORD  consists  of 2  required  cards 
and 3  optional  cards.    Then,  the  fourth  card  may  be  replaced  by  the  next  key-
word card.  All the fields in the omitted fourth and fifth cards are assigned their 
default values. 
WARNING:  In  this  example,  even  though  the  fourth  card  is  optional, 
the input deck may not jump from the third to fifth card.  
The only card that card 4 may be replaced with is the next 
keyword card. 
Long Format Input: 
To accommodate larger or more precise values for input variables than are allowed by 
the standard format input as described above, a “long format” input option is available.  
One  way  of  invoking  long  format  keyword  input  is  by  adding    “long=y”  to  the 
execution line.  A second way is to add “long=y” to the *KEYWORD command in the 
input deck. 
long=y: read long keyword input deck; write long structured input deck. 
long=s: read standard keyword input deck; write long structured input deck. 
long=k: read long keyword input deck; write standard structured input deck.
Getting Started 
The  “long=s”  option  may  be  helpful  in  the  rare  event  that  the  keyword  input  is  of 
standard format but LS-DYNA reports an input error and the dyna.str file   reveals  that  one  of  more  variables  is  incorrectly  written  to 
dyna.str as a series of asterisks due to inadequate field length(s) in dyna.str. 
The “long=k” option really serves no practical purpose. 
When long format is invoked for keyword input, field lengths for each variable become 
20  characters  long  (160  character  limit  per  line  for  8  variables;  200  character  limit  per 
line  for  10  variables).    In  this  way,  the  number  of  input  lines  in  long  format  is 
unchanged from regular format. 
To  convert  a  standard  format  input  deck  to  a  long  format  input  deck,  run  LS-DYNA 
with “newformat = long” on the execution line.  For example, if standard.k is a standard 
format input deck,  
ls-dyna i = standard.k newformat = long 
will create a long format input deck called standard.k.long. 
You can mix long and standard format within one input deck by use of “+” or “-“ signs 
within the deck.  If the execution line indicates standard format, you can add “ +” at the 
end  of  any  keywords  to  invoke  long  format  just  for  those  keywords.    For  example, 
“*NODE  +”  in  place  of  “*NODE”  invokes  a  read  format  of  two  lines  per  node  (I20, 
3E20.0 on the first line and 2F20.0 on the second line). 
Similarly, if the execution line indicates long format, you can add “-” at the end of any 
keywords to invoke standard format for those keywords.  For example, “*NODE –” in 
place  of  “*NODE”  invokes  the  standard  read  format  of  one  line  per  node  (I8,  3E16.0, 
2F8.0). 
Taking  this  idea  a  step  further,  adding  a  “-”  or  “+”  to  the  end  of  the  *INCLUDE 
keyword command signals to LS-DYNA that all the commands in the included file are 
standard format or long format, respectively.
Purpose:  Define an airbag or control volume. 
The keyword *AIRBAG provides a way of defining thermodynamic behavior of the gas 
flow into the airbag as well as a reference configuration for the fully inflated bag.  The 
keyword cards in this section are defined in alphabetical order: 
*AIRBAG_OPTION1_{OPTION2}_{OPTION3}_{OPTION4} 
*AIRBAG_ADVANCED_ALE 
*AIRBAG_ALE 
*AIRBAG_INTERACTION 
*AIRBAG_PARTICLE 
*AIRBAG_REFERENCE_GEOMETRY_OPTION_OPTION 
*AIRBAG_SHELL_REFERENCE_GEOMETRY
*AIRBAG_OPTION1_{OPTION2}_{OPTION3}_{OPTION4} 
OPTION1 specifies one of the following thermodynamic models: 
SIMPLE_PRESSURE_VOLUME 
SIMPLE_AIRBAG_MODEL 
ADIABATIC_GAS_MODEL 
WANG_NEFSKE 
WANG_NEFSKE_JETTING 
WANG_NEFSKE_MULTIPLE_JETTING 
LOAD_CURVE 
LINEAR_FLUID 
HYBRID 
HYBRID_JETTING   
HYBRID_CHEMKIN 
FLUID_AND_GAS 
OPTION2 specifies that an additional line of data is read for the WANG_NEFSKE type 
thermodynamic  relationships.    The  additional  data  controls  the  initiation  of  exit  flow 
from the airbag.  OPTION2 takes the single option: 
POP 
OPTION3  specifies  that  a  constant  momentum  formulation  is  used  to  calculate  the 
jetting load on the airbag an additional line of data is read in:  OPTION3 takes the single 
option: 
CM 
OPTION4 given by: 
ID 
Specifies that an airbag ID and heading information will be the first card of the airbag 
definition.    This  ID  is  a  unique  number  that  is  necessary  for  the  identification  of  the 
airbags  in  the  definition  of  airbag  interaction  via  *AIRBAG_INTERACTION  keyword.  
The numeric ID's and heading are written into the abstat and d3hsp files.
Core Cards: Common to all airbags 
ID Card.  Additional card for the ID keyword option.  To use the *AIRBAG_INTERAC-
TION keyword ID Cards are required.  
ID 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ABID 
Type 
I 
HEADING 
A70 
  Card 1a 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
SIDTYP 
RBID 
VSCA 
PSCA 
VINI 
MWD 
SPSF 
Type 
I 
Default 
none 
I 
0 
I 
0 
F 
1. 
F 
1. 
F 
0. 
F 
0. 
F 
0. 
Remark 
optional
  VARIABLE   
DESCRIPTION
ABID 
Airbag ID.  This must be a unique number. 
HEADING 
Airbag  descriptor.    It  is  suggested  that  unique  descriptions  be
used. 
SID 
Set ID 
SIDTYP 
Set type: 
EQ.0: segment, 
NE.0:  part set ID.
DESCRIPTION
*AIRBAG 
RBID 
Rigid body part ID for user defined activation subroutine: 
LT.0:  -RBID is taken as the rigid body part ID.  Built in sensor
subroutine  initiates  the  inflator.    Load  curves  are  offset
by initiation time. 
EQ.0: The control volume is active from time zero. 
GT.0:  RBID  is  taken  as  the  rigid  body  part  ID.    User  sensor
subroutine  initiates  the  inflator.    Load  curves  are  offset
by initiation time.  See Appendix D. 
Volume scale factor  (default = 1.0) 
Pressure scale factor (default = 1.0) 
Initial filled volume 
Mass weighted damping factor, D 
Stagnation pressure scale factor, 0 <= 𝛾 <= 1 
VSCA 
PSCA 
VINI 
MWD 
SPSF 
Remarks: 
The first card is necessary for all airbag options.  The option dependent cards follow. 
Lumped  parameter  control  volumes  are  a  mechanism  for  determining  volumes  of 
closed  surfaces  and  applying  a  pressure  based  on  some  thermodynamic  relation.    The 
volume  is  specified  by  a  list  of  polygons  similar  to  the  pressure  boundary  condition 
cards or by specifying a material subset which represents shell elements which form the 
closed  boundary.    All  polygon  normal  vectors  must  be  oriented  to  face  outwards  from 
the control volume, however for *AIRBAG_PARTICLE, which does not rely on control 
volumes,  all  polygon  normal  vectors  must  be  oriented  to  face  inwards  to  get  proper 
volume .  If holes are detected, they are 
assumed to be covered by planar surfaces. 
There  are  two  sets  of  volume  and  pressure  variables  used  for  each  control  volume 
model.    First,  the  finite  element  model  computes  a  volume  𝑉femodel  and  applies  a 
pressure  𝑃femodel.    The  thermodynamics  of  a  control  volume  may  be  computed  in  a 
different  unit  system  with  its  own  set  of  varriables:  𝑉cvolume  and  pressure  𝑃cvolume 
which  are  used  for  integrating  the  differential  equations  for  the  control  volume.    The 
conversion is as follows: 
𝑉cvolume = (VSCA × 𝑉femodel) − VINI 
𝑃femodel = PSCA×𝑃cvolume
Where  VSCA,  PSCA, and  VINI  are  input  parameters.    Damping  can  be  applied  to  the 
structure enclosing a control volume by using a mass weighted damping formula: 
𝑑 = 𝑚𝑖𝐷(𝑣𝑖 − 𝑣cg) 
𝐹𝑖
𝑑 is the damping force, mi is the nodal mass, 𝜈𝑖 is the velocity for a node, 𝑣cg is 
where 𝐹𝑖
the mass weighted average velocity of the structure enclosing the control volume, and 
D is the damping factor. 
An alternative, separate damping is based on the stagnation pressure.  The stagnation 
pressure is roughly the maximum pressure on a flat plate oriented normal to a steady 
state flow field.  The stagnation pressure is defined as 𝑝 = 𝛾𝜌𝑉2 where 𝑉 is the normal 
velocity  of  the  control  volume  relative  to  the  ambient  velocity,  𝜌  is  the  ambient  air 
density,  and  𝛾  is  a  factor  which  varies  from  0  to  1  and  has  to  be  chosen  by  the  user.  
Small values are recommended to avoid excessive damping. 
Sensor input: 
The sensor is mounted on a rigid body which is attached to the structure.  The motion of 
the sensor is evaluated in the local coordinate system of the rigid body.  See *MAT_RIGID.  This 
local system rotates and translates with the rigid material.  The default local system for 
a rigid body is taken as the principal axes of the inertia tensor. 
When  the  user  defined  criterion  for  airbag  deployment  is  satisfied,  a  flag  is  set  and 
deployment begins.  All load curves relating to the mass flow rate versus time are then 
shifted by the initiation time. 
RBID = 0: No rigid body 
For  this  case  there  is  no  rigid  body,  and  the  control  volume  is  active  from  time  zero.  
There are no additional sensor cards. 
RBID > 0: User supplied sensor subroutine 
The  value  of  RBID  is  taken  as  a  rigid  body  part  ID,  and  a  user  supplied  sensor 
subroutine will be called to determine the flag that initiates deployment.  See Appendix 
D for details regarding the user supplied subroutine.  For RBID > 0 the additional cards 
are specified below:
User Subroutine Control Card.  This card is read in when RBID > 0. 
2 
3 
4 
5 
6 
7 
8 
  Card 1b 
Variable 
Type 
1 
N 
I 
Default 
none 
User  Subroutine  Constant  Cards.    Define  N  constants  for  the  user  subroutine. 
Include only the number of cards necessary, i.e.  for nine constants use 2 cards. 
  Card 1c 
Variable 
1 
C1 
Type 
F 
Default 
0. 
2 
C2 
F 
0. 
3 
C3 
F 
0. 
4 
C4 
F 
0. 
5 
C5 
F 
0. 
6 
7 
8 
  VARIABLE   
DESCRIPTION
N 
Number of input parameters (not to exceed 25). 
C1, …, CN 
Up to 25 constants for the user subroutine. 
RBID < 0: User supplied sensor subroutine 
The  value  of  –RBID  is  taken  as  rigid  body  part  ID  and  a  built  in  sensor  subroutine  is 
called.  For RBID < 0 there are three additional cards.
Acceleration Sensor Card. 
  Card 1d 
Variable 
1 
AX 
Type 
F 
Default 
0. 
2 
AY 
F 
0. 
3 
AZ 
F 
0. 
Velocity Sensor Card. 
4 
5 
6 
7 
8 
AMAG 
TDUR 
F 
0. 
F 
0. 
  Card 1e 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DVX 
DVY 
DVZ 
DVMAG 
Type 
F 
Default 
0. 
F 
0. 
Displacement Sensor Card. 
  Card 1f 
Variable 
1 
UX 
Type 
F 
Default 
0. 
2 
UY 
F 
0. 
F 
0. 
3 
UZ 
F 
0. 
F 
0. 
4 
5 
6 
7 
8 
UMAG 
F 
0.
AX 
AY 
AZ 
*AIRBAG 
DESCRIPTION
Acceleration  level  in  local  𝑥-direction  to  activate  inflator.    The 
absolute value of the 𝑥-acceleration is used. 
EQ.0: inactive. 
Acceleration  level  in  local  𝑦-direction  to  activate  inflator.    The 
absolute value of the 𝑦-acceleration is used. 
EQ.0: inactive. 
Acceleration  level  in  local  𝑧-direction  to  activate  inflator.    The 
absolute value of the 𝑧-acceleration is used. 
EQ.0: inactive. 
AMAG 
Acceleration magnitude required to activate inflator. 
EQ.0: inactive. 
TDUR 
DVX 
DVY 
DVZ 
Time  duration  acceleration  must  be  exceeded  before  the  inflator
activates.    This  is  the  cumulative  time  from  the  beginning  of  the
calculation, i.e., it is not continuous. 
Velocity  change  in  local 𝑥-direction  to  activate  the  inflator.    (The 
absolute value of the velocity change is used.) 
EQ.0: inactive. 
Velocity  change  in  local 𝑦-direction  to  activate  the  inflator.    (The 
absolute value of the velocity change is used.) 
EQ.0: inactive. 
Velocity  change  in  local  𝑧-direction  to  activate  the  inflator.    (The 
absolute value of the velocity change is used.) 
EQ.0: inactive. 
DVMAG 
Velocity change magnitude required to activate the inflator.   
EQ.0: inactive. 
UX 
Displacement  increment  in  local  𝑥-direction  to  activate  the 
inflator.  (The absolute value of the 𝑥-displacement is used.) 
EQ.0: inactive.
UY 
UZ 
*AIRBAG 
DESCRIPTION
Displacement  increment  in  local  𝑦-direction  to  activate  the 
inflator.  (The absolute value of the 𝑦-displacement is used.) 
EQ.0: inactive. 
Displacement  increment  in  local  𝑧-direction  to  activate  the 
inflator.  (The absolute value of the 𝑧-displacement is used.) 
EQ.0: inactive. 
UMAG 
Displacement magnitude required to activate the inflator. 
EQ.0: inactive.
*AIRBAG_SIMPLE_PRESSURE_VOLUME_OPTION 
Additional  card  for  SIMPLE_PRESSURE_VOLUME  option.    (For  card  1  see  the  “core 
cards” section of *AIRBAG.) 
  Card 2 
Variable 
1 
CN 
2 
3 
4 
5 
6 
7 
8 
BETA 
LCID 
LCIDDR 
Type 
F 
F 
I 
Default 
none 
none 
none 
I 
0 
  VARIABLE   
DESCRIPTION
CN 
Coefficient.  Define if the load curve ID, LCID, is unspecified. 
LT.0.0: |CN| is the load curve ID, which defines the coefficient
as a function of time. 
Scale factor, 𝛽.  Define if a load curve ID is not specified. 
Optional load curve ID defining pressure versus relative volume.
Optional load curve ID defining the coefficient, CN, as a function
of time during the dynamic relaxation phase. 
BETA 
LCID 
LCIDDR 
Remarks: 
The relationship is the following: 
Pressure =
𝛽 × CN
Relative  Volume
Relative  Volume =
Current  Volume
Initial  Volume
The pressure is then a function of the ratio of current volume to the initial volume.  The 
constant,  CN,  is  used  to  establish  a  relationship  known  from  the  literature.    The  scale 
factor 𝛽 is simply used to scale the given values.  This simple model can be used when 
an initial pressure is given and no leakage, no temperature, and no input mass flow is 
assumed.  A typical application is the modeling of air in automobile tires. 
The  load  curve,  LCIDDR,  can  be  used  to  ramp  up  the  pressure  during  the  dynamic 
relaxation phase in order to avoid oscillations after the desired gas pressure is reached.
In the DEFINE_CURVE section this load curve must be flagged for dynamic relaxation.  
After initialization either the constant or load curve ID, |CN| is used to determine the 
pressure.
*AIRBAG_SIMPLE_AIRBAG_MODEL_OPTION 
Additional  cards  for  SIMPLE_AIRBAG_MODEL  option.    (For  card  1  see  the  “core 
cards” section of *AIRBAG.) 
  Card 2 
Variable 
1 
CV 
Type 
F 
2 
CP 
F 
3 
T 
F 
4 
5 
6 
LCID 
MU 
AREA 
I 
F 
F 
7 
PE 
F 
8 
RO 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 3 
1 
2 
Variable 
LOU 
T_EXT 
Type 
Default 
Remarks 
I 
0 
0 
F 
0. 
3 
A 
F 
4 
B 
F 
0. 
0. 
5 
6 
7 
8 
MW 
GASC 
F 
0. 
F 
0. 
optional  optional optional optional optional 
  VARIABLE   
DESCRIPTION
CV 
CP 
T 
LCID 
Heat capacity at constant volume, e.g., Joules/kg/oK. 
Heat capacity at constant pressure, e.g., Joules/kg/oK. 
Temperature of input gas 
Load  curve  ID  specifying  input  mass  flow  rate.    See  *DEFINE_-
CURVE. 
MU 
Shape factor for exit hole, 𝜇: 
LT.0.0: ∣𝜇∣ is the load curve number defining the shape factor as
a function of absolute pressure.
VARIABLE   
DESCRIPTION
AREA 
Exit area, A: 
GE.0.0: A is the exit area and is constant in time, 
LT.0.0:  |A| is the load curve number defining the exit area as
a function of absolute pressure. 
PE 
RO 
LOU 
Ambient pressure, 𝑝𝑒 
Ambient density, 𝜌 
Optional  load  curve  ID  giving  mass  flow  out  versus  gauge
pressure in bag.  See *DEFINE_CURVE. 
Leave the following 5 fields blank blank if CV ≠ 0 
T_EXT 
Ambient temperature. 
First  heat 
Joules/mole/oK). 
capacity 
Second  heat 
Joules/mole/oK2). 
capacity 
coefficient 
of 
inflator  gas 
(e.g.,
coefficient  of 
inflator  gas, 
(e.g.,
Molecular weight of inflator gas (e.g., Kg/mole). 
Universal 
Joules/mole/oK). 
gas 
constant 
of 
inflator 
gas 
(e.g., 
8.314
A 
B 
MW 
GASC 
Remarks: 
The gamma law equation of state used to determine the pressure in the airbag: 
𝑝 = (𝛾 − 1)𝜌𝑒 
where p is the pressure, 𝜌 is the density, 𝑒 is the specific internal energy of the gas, and 𝛾 
is the ratio of the specific heats: 
𝛾 =
𝑐𝑝
𝑐𝑣
From conservation of mass, the time rate of change of mass flowing into the bag is given 
as: 
𝑑𝑀
𝑑𝑡
=
𝑑𝑀in
𝑑𝑡
−
𝑑𝑀out
𝑑𝑡
The inflow mass flow rate is given by the load curve ID, LCID.  Leakage, the mass flow 
rate out of the bag, can be modeled in two alternative ways.  One is to give an exit area 
with the corresponding shape factor, then the load curve ID, LOU, must be set to zero.  
The other is to define a mass flow out by a load curve, then 𝜇 and A have to both be set 
to zero. 
If CV = 0.  then the constant-pressure specific heat is given by: 
and the constant-volume specific heat is then found from: 
𝑐𝑝 =
(𝑎 + 𝑏𝑇)
MW
𝑐𝑣 = 𝑐𝑝 −
MW
*AIRBAG_ADIABATIC_GAS_MODEL_OPTION 
Additional  card  for  ADIABATIC_GAS_MODEL  option.    (For  card  1  see  the  “core 
cards” section of *AIRBAG.) 
  Card 2 
1 
2 
3 
Variable 
PSF 
LCID 
GAMMA 
Type 
F 
I 
F 
4 
P0 
F 
5 
PE 
F 
6 
RO 
F 
7 
8 
Default 
1.0 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
PSF 
LCID 
Pressure scale factor 
Optional load curve for preload flag.  See *DEFINE_CURVE. 
GAMMA 
Ratio of specific heats 
P0 
PE 
RO 
Initial pressure (gauge) 
Ambient pressure 
Initial density of gas 
Remarks: 
The optional load curve ID, LCID, defines a preload flag.  During the preload phase the 
function  value  of  the  load  curve  versus  time  is  zero,  and  the  pressure  in  the  control 
volume is given as:  
𝑝 = PSF × 𝑝0 
When the first nonzero function value is encountered, the preload phase stops and the 
ideal  gas  law  applies  for  the  rest  of  the  analysis.    If  LCID  is  zero,  no  preload  is 
performed. 
The gamma law equation of state for the adiabatic expansion of an ideal gas is used to 
determine the pressure after preload: 
𝑝 = (𝛾 − 1)𝜌𝑒 
where p is the pressure, 𝜌 is the density, e  is the specific internal energy of the gas, and 
𝛾 is the ratio of the specific heats:
𝛾 =
𝑐𝑝
𝑐𝑣
The pressure above is the absolute pressure, the resultant pressure acting on the control 
volume is: 
𝑝𝑠 = PSF × (𝑝 − 𝑝𝑒) 
where  PSF  is  the  pressure  scale  factor.    Starting  from  the  initial  pressure  𝑝0  an  initial 
internal energy is calculated: 
𝑒0 =
𝑝0 + 𝑝𝑒
𝜌(𝛾 − 1)
*AIRBAG 
The following sequence of cards is read in for the all variations of the WANG_NEFSKE 
option to *AIRBAG.  For card 1 see the “core cards” section of *AIRBAG. 
  Card 2 
Variable 
1 
CV 
Type 
F 
2 
CP 
F 
3 
T 
F 
Default 
none 
none 
0. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
LCT 
LCMT 
TVOL 
LCDT 
IABT 
I 
0 
4 
I 
F 
I 
F 
none 
0. 
0. 
not used
5 
6 
7 
8 
Variable 
C23 
LCC23 
A23 
LCA23 
CP23 
LCCP23 
AP23 
LCAP23 
Type 
F 
Default 
none 
  Card 4 
Variable 
1 
PE 
Type 
F 
I 
0 
2 
RO 
F 
F 
none 
3 
GC 
F 
Default 
none 
none 
none 
I 
0 
4 
F 
none 
5 
I 
0 
6 
F 
0.0 
7 
I 
0 
8 
LCEFR 
POVER 
PPOP 
OPT 
KNKDN 
I 
0 
F 
F 
F 
0.0 
0.0 
0.0 
I
Inflator  Card.    If  the  inflator  is  modeled,  LCMT = 0  fill  in  the  following  card.    If  not, 
include but leave blank. 
  Card 5 
1 
2 
3 
4 
Variable 
IOC 
IOA 
IVOL 
IRO 
Type 
F 
F 
F 
F 
5 
IT 
F 
6 
7 
8 
LCBF 
I 
Default 
none 
none 
none 
none 
none 
none 
Temperature Dependent Heat Capacities Card.  Include this card when CV = 0.  
  Card 6 
1 
Variable 
TEXT 
Type 
F 
2 
A 
F 
3 
B 
F 
4 
5 
6 
7 
8 
MW 
GASC 
HCONV 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
Criteria  for  Initiating  Exit  Flow  Card.    Additional  card  for  the  POP  option  to  the 
*AIRBAG_WANG_NEFSKE card.  
  Card 7 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TDP 
AXP 
AYP 
AZP 
AMAGP 
TDURP 
TDA 
RBIDP 
Type 
F 
F 
F 
F 
F 
F 
F 
I 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
none 
  VARIABLE   
DESCRIPTION
CV 
CP 
T 
Specific heat at constant volume, e.g., Joules/kg/oK. 
Specific heat at constant pressure, e.g., Joules/kg/oK. 
Temperature  of  input  gas.    For  temperature  variations  a  load
curve, LCT, may be defined.
VARIABLE   
DESCRIPTION
LCT 
LCMT 
TVOL 
LCDT 
IABT 
C23 
LCC23 
A23 
LCA23 
Optional  load  curve  number  defining  temperature  of  input  gas
versus time.  This overrides columns T. 
Load  curve  specifying  input  mass  flow  rate  or  tank  pressure
versus time.  If the tank volume, TVOL, is nonzero the curve ID is
assumed to be tank pressure versus time.   If LCMT = 0, then the 
inflator  has  to  be  modeled,  see  Card  5.    During  the  dynamic
relaxation phase the airbag is ignored unless the curve is flagged
to act during dynamic relaxation. 
Tank volume which is required only for the tank pressure versus
time curve, LCMT. 
Load curve for time rate of change of temperature (dT/dt) versus
time. 
Initial airbag temperature.  (Optional, generally not defined.) 
Vent  orifice  coefficient  which  applies  to  exit  hole.    Set  to  zero  if
LCC23 is defined below. 
The  absolute  value,  |LCC23|,  is  a  load  curve  ID.    If  the  ID  is
positive, the load curve defines the vent orifice coefficient which
applies to exit hole as a function of time.  If the ID is negative, the
vent  orifice  coefficient  is  defined  as  a  function  of  relative
pressure, 𝑃air/𝑃bag, see [Anagonye and Wang 1999].  In addition,
LCC23  can  be  defined  through  *DEFINE_CURVE_FUNCTION. 
A nonzero value for C23 overrides LCC23.   
If defined as a positive number, A23 is the vent orifice area which
applies to exit hole.  If defined as a negative number, the absolute
value  |A23|  is  a  part  ID,  see  [Anagonye  and  Wang,  1999].    The
area  of  this  part  becomes  the  vent  orifice  area.    Airbag  pressure 
will  not  be  applied  to  part  |A23|  representing  venting  holes  if
part  |A23|  is  not  included  in  SID,  the  part  set  representing  the
airbag.  Set A23 to zero if LCA23 is defined below. 
Load  curve  number  defining  the  vent  orifice  area  which  applies 
to  exit  hole  as  a  function  of  absolute  pressure,  or  LCA23  can  be 
defined  through  *DEFINE_CURVE_FUNCTION.    A  nonzero 
value for A23 overrides LCA23. 
CP23 
Orifice  coefficient  for  leakage  (fabric  porosity).    Set  to  zero  if
LCCP23 is defined below.
LCCP23 
*AIRBAG_WANG_NEFSKE 
DESCRIPTION
Load  curve  number  defining  the  orifice  coefficient  for  leakage
(fabric porosity) as a function of time, or LCCP23 can be defined 
through  *DEFINE_CURVE_FUNCTION.    A  nonzero  value  for 
CP23 overrides LCCP23. 
AP23 
Area for leakage (fabric porosity) 
LCAP23 
PE 
RO 
GC 
Load curve number defining the area for leakage (fabric porosity)
as  a  function  of  (absolute)  pressure,  or  LCAP23  can  be  defined
through  *DEFINE_CURVE_FUNCTION.    A  nonzero  value  for 
AP23 overrides LCAP23. 
Ambient pressure 
Ambient density 
Gravitational  conversion  constant  (mandatory  -  no  default).    If 
consistent  units  are  being  used  for  all  parameters  in  the  airbag
definition then unity should be input. 
LCEFR 
Optional  curve  for  exit  flow  rate  (mass/time)  versus  (gauge)
pressure 
POVER 
Initial relative overpressure (gauge), Pover in control volume 
PPOP 
OPT 
Pop  Pressure:  relative  pressure  (gauge)  for  initiating  exit  flow,
Ppop 
Fabric  venting  option,  if  nonzero  CP23,  LCCP23,  AP23,  and
LCAP23 are set to zero. 
EQ.1: Wang-Nefske formulas for venting through an orifice are 
used.  Blockage is not considered. 
EQ.2: Wang-Nefske formulas for venting through an orifice are
used.  Blockage of venting area due to contact is consid-
ered. 
EQ.3: Leakage  formulas  of  Graefe,  Krummheuer,  and  Siejak
[1990] are used.  Blockage is not considered. 
EQ.4: Leakage  formulas  of  Graefe,  Krummheuer,  and  Siejak
[1990] are used.  Blockage of venting area due to contact
is considered. 
EQ.5: Leakage formulas based on flow through a porous media
are used.  Blockage is not considered.
VARIABLE   
DESCRIPTION
EQ.6: Leakage formulas based on flow through a porous media
are used.  Blockage of venting area due to contact is con-
sidered.   
EQ.7: Leakage is based on gas volume outflow versus pressure 
load  curve.    Blockage  of  flow  area  due  to  contact  is  not
considered.    Absolute  pressure  is  used  in  the  porous-
velocity-versus-pressure  load  curve,  given  as  FAC(P)  in 
the *MAT_FABRIC card. 
EQ.8: Leakage is based on gas volume outflow versus pressure 
load curve.  Blockage of flow area due to contact is con-
sidered.    Absolute  pressure  is  used  in  the  porous-
velocity-versus-pressure  load  curve,  given  as  FAC(P)  in 
the *MAT_FABRIC card. 
Optional  load  curve  ID  defining  the  knock  down  pressure  scale 
factor versus time.  This option only applies to jetting.  The scale
factor  defined  by  this  load  curve  scales  the  pressure  applied  to
airbag segments which 
do not have a clear line-of-sight to the jet.  Typically, at very early 
times this scale factor will be less than unity and equal to unity at
later  times.    The  full  pressure  is  always  applied  to  segments
which can see the jets. 
KNKDN 
IOC 
IOA 
Inflator orifice coefficient 
Inflator orifice area 
IVOL 
Inflator volume 
IRO 
IT 
LCBF 
TEXT 
A 
B 
Inflator density 
Inflator temperature 
Load curve defining burn fraction versus time 
Ambient temperature. 
First  molar  heat  capacity  coefficient  of 
Joules/mole/oK) 
inflator  gas  (e.g.,
Second  molar  heat  capacity  coefficient  of  inflator  gas,  (e.g.,
Joules/mole/oK2)
MW 
GASC 
HCONV 
*AIRBAG_WANG_NEFSKE 
DESCRIPTION
Molecular weight of inflator gas (e.g., Kg/mole). 
Universal gas constant of inflator gas (e.g., 8.314 Joules/mole/oK)
Effective  heat  transfer  coefficient  between  the  gas  in  the  air  bag
and the environment at temperature TEXT.  If HCONV < 0, then 
HCONV defines a load curve of data pairs (time, hconv). 
TDP 
Time  delay  before  initiating  exit  flow  after  pop  pressure  is
reached. 
AXP 
Pop acceleration magnitude in local x-direction. 
EQ.0.0: Inactive. 
AYP 
Pop acceleration magnitude in local y-direction. 
EQ.0.0: Inactive. 
AZP 
Pop acceleration magnitude in local z-direction. 
EQ.0.0: Inactive. 
AMAGP 
Pop acceleration magnitude. 
EQ.0.0: Inactive. 
Time  duration  pop  acceleration must  be  exceeded  to  initiate  exit
flow.    This  is  a  cumulative  time  from  the  beginning  of  the
calculation, i.e., it is not continuous. 
Time  delay  before  initiating  exit  flow  after  pop  acceleration  is 
exceeded for the prescribed time duration. 
Part  ID  of  the  rigid  body  for  checking  accelerations  against  pop
accelerations. 
TDURP 
TDA 
RBIDP 
Remarks: 
The gamma law equation of state for the adiabatic expansion of an ideal gas is used to 
determine the pressure after preload: 
𝑝 = (𝛾 − 1)𝜌𝑒 
where p is the pressure, 𝜌  is the density, e  is the specific internal energy of the gas, and 
𝛾 is the ratio of the specific heats:
𝛾 =
𝑐𝑝
𝑐𝑣
where cv is the specific heat at constant volume, and cp is the specific heat at constant 
pressure.  A pressure relation is defined: 
𝑄 =
𝑝𝑒
where  pe  is  the  external  pressure  and  p  is  the  internal  pressure  in  the  bag.    A  critical 
pressure relationship is defined as: 
𝑄crit = (
𝛾 + 1
𝛾−1
)
where 𝛾 is the ratio of specific heats: 
and 
𝛾 =
𝑐𝑝
𝑐𝑣
𝑄 ≤ 𝑄crit⇒𝑄 = 𝑄crit. 
Wang and Nefske define the mass flow through the vents and leakage by 
and 
𝑚̇ 23 = 𝐶23𝐴23
𝑅√𝑇2
𝛾√2𝑔𝑐 (
𝛾𝑅
𝛾 − 1
) (1 − 𝑄
𝛾−1
𝛾 ) 
𝑚′̇
23 = 𝐶′23𝐴′23
𝑅√𝑇2
𝛾√2𝑔𝑐 (
𝛾𝑅
𝛾 − 1
) (1 − 𝑄
𝛾−1
𝛾 ) 
It must be noted that the gravitational conversion constant has to be given in consistent 
units.  As an alternative to computing the mass flow out of the bag by the Wang-Nefske 
model, a curve for the exit flow rate depending on the internal pressure can be taken.  
Then,  no  definitions  for  C23,  LCC23,  A23,  LCA23,  CP23,  LCCP23,  AP23,  and  LCAP23 
are necessary. 
The airbag inflator assumes that the control volume of the inflator is constant and that 
the  amount  of  propellant  reacted  can  be  defined  by  the  user  as  a  tabulated  curve  of 
fraction reacted versus time.  A pressure relation is defined: 
𝑄crit =
𝑝𝑐
𝑝𝑖
= (
𝛾 + 1
𝛾−1
)
where  𝑝𝑐  is  a  critical  pressure  at  which  sonic  flow  occurs,  𝑝𝐼,  is  the  inflator  pressure.  
The exhaust pressure is given by
𝑝𝑒 = {
𝑝𝑎
𝑝𝑐
if 𝑝𝑎 ≥ 𝑝𝑐
if 𝑝𝑎 < 𝑝𝑐
where 𝑝𝑎 is the pressure in the control volume.  The mass flow into the control volume 
is governed by the equation: 
√
√
√
√
𝑔𝑐𝛾 (𝑄
𝛾 − 𝑄
𝛾+1
𝛾 )
𝑚̇ in = 𝐶0𝐴0√2𝑝𝐼𝜌𝐼
⎷
where  𝐶0,  𝐴0,  and  𝜌𝐼    are  the  inflator  orifice  coefficient,  area,  and  gas  density, 
respectively. 
𝛾 − 1
If OPT is defined, then for OPT set to 1 or 2 the mass flow rate out of the bag, 𝑚̇ 𝑜𝑢𝑡 is 
given by: 
nairmats
𝑚̇ 𝑜𝑢𝑡 = √𝑔𝑐 { ∑ [FLC(𝑡)𝑛 × FAC(𝑝)𝑛 × Area𝑛]
} √2𝑝𝜌
𝑛=1
√
√
√
√
⎷
𝑘 − 𝑄
𝛾+1
𝛾 )
𝛾 (𝑄
𝛾 − 1
where,  𝜌  is  the  density  of  airbag  gas,  “nairmats”  is  the  number  of  fabrics  used  in  the 
airbag, and “Arean” is the current unblocked area of fabric number n. 
If OPT set to 3 or 4 then: 
nairmats
𝑚̇ out = { ∑ [FLC(𝑡)𝑛 × FAC(𝑝)𝑛 × Area𝑛]
} √2(𝑝 − 𝑝ext)𝜌 
and for OPT set to 5 or 6: 
𝑛=1
nairmats
𝑚̇ out = { ∑ [FLC(𝑡)𝑛 × FAC(𝑝)𝑛 × Area𝑛]
} (𝑝 − 𝑝ext) 
𝑛=1
and for OPT set to 7 or 8 (may be comparable to an equivalent model ALE model): 
nairmats
𝑚̇ out = ∑ FLC(𝑡)𝑛×FAC(𝑝)𝑛 × Area𝑛 × 𝜌𝑛
𝑛=1
Note  that  for  different  OPT  settings, FAC(𝑝)𝑛  has  different  meanings  (all  units  shown 
just as demonstrations): 
1.  For OPT of 1, 2, 3 and 4, FAC(P) is unit-less. 
2.  For OPT of 5 and 6, FAC(P) has a unit of (s/m). 
3.  For  OPT  of  7  or  8,  FAC(P)  is  the  gas  volume  outflow  through  a  unit  area  per 
unit time thus has the unit of speed, 
4. 
[FAC(𝑃)] = [volume]
[area][𝑡] = [L]3
[L]2[𝑡]
= [𝐿]
[𝑡] = [velocity].
Multiple  airbags  may  share  the  same  part  ID  since  the  area  summation  is  over  the 
airbag segments whose corresponding part ID’s are known.  Currently, we assume that 
no more than ten materials are used per bag for purposes of the output.  This constraint 
can be eliminated if necessary. 
The total mass flow out will include the portion due to venting, i.e., constants C23 and 
A23 or their load curves above. 
If CV = 0.  then the constant-pressure specific heat is given by:  
and the constant-volume specific heat is then found from: 
𝑐𝑝 =
(𝑎 + 𝑏𝑇)
𝑀𝑊
𝑐𝑣 = 𝑐𝑝 −
𝑀𝑊
Two additional cards are required for JETTING models: 
The  following  additional  cards  are  defined  for  the  WANG_NEFSKE_JETTING  and 
WANG_NEFSKE_MULTIPLE_JETTING options, two further cards are defined for each 
option.  The jet may be defined by specifying either the coordinates of the jet focal point, 
jet  vector  head  and  secondary  jet  focal  point,  or  by  specifying  three  nodes  located  at 
these  positions.    The  nodal  point  option  is  recommended  when  the  location  of  the 
airbag changes as a function of time. 
NOTE:  For Jetting models define either of the two cards be-
low but not both. 
Card format 8 for WANG_NEFSKE keyword option. 
  Card 8 
1 
2 
3 
4 
5 
6 
Variable 
XJFP 
YJFP 
ZJFP 
XJVH 
YJVH 
ZJVH 
Type 
F 
F 
F 
F 
F 
F 
7 
CA 
F 
8 
BETA 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
1.0 
Remark 
1 
1 
1 
1 
1
Card format 8 for WANG_NEFSKE_MUTTIPLE_JETTING keyword options. 
  Card 8 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
XJFP 
YJFP 
ZJFP 
XJVH 
YJVH 
ZJVH 
LCJRV 
BETA 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
1.0 
Remark 
1 
1 
1 
1 
1 
1 
Card  9  for  both  WANG_NEFSKE_JETTING  and  WANG_NEFSKE_MULTIPLE_JET-
TING. 
  Card 9 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
XSJFP 
YSJFP 
ZSJFP 
PSID 
ANGLE 
NODE1 
NODE2 
NODE3 
Type 
F 
F 
F 
I 
F 
Default 
none 
none 
none 
none 
none 
Remark 
I 
0 
1 
I 
0 
1 
I 
0
Airbag
Gaussian velocity profile
Virtual origin
Node 1
Node 2
Hole diameter
Pressure is applied to surfaces
that are in the line of sight of
the virtual origin.
α: smaller
α: larger
Figure  3-1.    Jetting  configuration  for  driver's  side  airbag  (pressure  applied
only if centroid of surface is in line-of-sight) 
Secondary focal jet point
Virtual origin
Node 1
Node 3
Gaussian profile
Node 2
Figure 3-2.  Jetting configuration for the passenger’s side bag. 
  VARIABLE   
DESCRIPTION
XJFP 
YJFP 
x-coordinate of jet focal point, i.e., the virtual origin in Figures 3-1
and 3-2.  See Remark 1 below. 
y-coordinate of jet focal point, i.e., the virtual origin in Figures 3-1
and 3-2.
Relative jet
velocity
(degrees)
cut off angle, ψ
for ψ > ψ
cut v=0
cut
Figure 3-3.  Normalized jet velocity versus angle for multiple jet driver's side
airbag 
  VARIABLE   
DESCRIPTION
ZJFP 
XJVH 
YJVH 
ZJVH 
CA 
LCJRV 
z-coordinate of jet focal point, i.e., the virtual origin in Figures 3-1
and 3-2. 
x-coordinate of jet vector head to defined code centerline 
y-coordinate of jet vector head to defined code centerline 
z-coordinate of jet vector head to defined code centerline 
Cone angle, 𝛼, defined in radians. 
LT.0.0: |𝛼| is the load curve ID defining cone angle as a function
of time 
Load curve ID giving the spatial jet relative velocity distribution,
see Figures 3-1, 3-2, and 3-3.  The jet velocity is determined from 
the inflow mass rate and scaled by the load curve function value
corresponding  to  the value  of  the  angle  𝜓.    Typically,  the  values 
on  the  load  curve  vary  between  0  and  unity.    See  *DEFINE_-
CURVE. 
BETA 
Efficiency  factor,  𝛽,  which  scales  the  final  value  of  pressure 
obtained from Bernoulli’s equation. 
LT.0.0: ∣𝛽∣ is the load curve ID defining the efficiency factor as a
function of time
cut
Figure  3-4.    Multiple  jet  model  for  driver's  side  airbag.    Typically,  𝜓cut   is close to 90°.  The angle 𝜓0 is included to indicate that there is
some angle below which the jet is negligible; see Figure 3-3. 
  VARIABLE   
XSJFP 
YSJFP 
ZSJFP 
PSID 
ANGLE 
DESCRIPTION
x-coordinate of secondary jet focal point, passenger side bag.  If
the coordinates of the secondary point are (0,0,0) then a conical
jet (driver’s side airbag) is assumed. 
y-coordinate of secondary jet focal point 
z-coordinate of secondary jet focal point 
Optional  part  set  ID,  see  *SET_PART.    If  zero  all  elements  are 
included in the airbag. 
Cutoff  angle  in  degrees.    The  relative  jet  velocity  is  set  to  zero 
for  angles  greater  than  the  cutoff.    See  Figure  3-3.    This  option 
applies to the MULTIPLE jet only. 
NODE1 
Node  ID  located  at  the  jet  focal  point,  i.e.,  the  virtual  origin  in 
Figures 3-1 and 3-2.  See Remark 1 below. 
NODE2 
Node ID for node along the axis of the jet. 
NODE3 
Optional node ID located at secondary jet focal point.
*AIRBAG_WANG_NEFSKE 
1. 
It  is  assumed  that the jet  direction  is  defined  by  the  coordinate  method  (XJFP, 
YJFP,  ZJFP)  and  (XJVH,  YJVH,  ZJVH)  unless  both  NODE1  and  NODE2  are 
defined.    In  which  case  the  coordinates  of  the  nodes  give  by  NODE1,  NODE2 
and  NODE3  will  override  (XJFP,  YJFP,  ZJFP)  and  (XJVH,  YJVH,  ZJVH).    The 
use  of  nodes  is  recommended  if  the  airbag  system  is  undergoing  rigid  body 
motion.    The  nodes  should  be  attached  to  the  vehicle  to  allow  for  the  coordi-
nates of the jet to be continuously updated with the motion of the vehicle. 
2.  The  jetting  option  provides  a  simple  model  to  simulate  the  real  pressure 
distribution in the airbag during the breakout and early unfolding phase.  Only 
the surfaces that are in the line of sight to the virtual origin have an increased 
pressure  applied.    With  the  optional  load  curve  LCRJV,  the  pressure  distribu-
tion with the code can be scaled according to the so-called relative jet velocity 
distribution.   
3.  For  passenger  side  airbags  the  cone  is  replaced  by  a  wedge  type  shape.    The 
first  and  secondary  jet  focal  points  define  the  corners  of  the  wedge  and  the 
angle 𝛼 then defines the wedge angle. 
4. 
Instead  of  applying  pressure  to  all  surfaces  in  the  line  of  sight  of  the  virtual 
origin(s), a part set can be defined to which the pressure is applied.  
5.  Care must be used to place the jet focal point within the bag.  If the focal point 
is outside the bag, inside surfaces will not be visible so jetting pressure will not 
be applied correctly.
Additional card required for CM option: 
The  following  additional  card  is  defined  for  the  WANG_NEFSKE_JETTING_CM  and 
WANG_NEFSKE_MULTIPLE_JETTING_CM options. 
Additional card required for CM keyword option. 
  Card 10 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NREACT 
Type 
I 
Default 
none 
Remark 
  VARIABLE   
NREACT 
Remarks: 
DESCRIPTION
Node  for  reacting  jet  force.    If  zero  the  jet  force  will  not  be
applied. 
Compared  with  the  standard  LS-DYNA  jetting  formulation,  the  Constant  Momentum 
option has several differences.  Overall, the jetting usually has a more significant effect 
on  airbag  deployment  than  the  standard  LS-DYNA  jetting:  the  total  force  is  often 
greater, and does not reduce with distance from the jet. 
The velocity at the jet outlet is assumed to be a choked (sonic) adiabatic flow of a perfect 
gas.  Therefore the velocity at the outlet is given by: 
𝑣outlet = √𝛾𝑅𝑇 = √
(𝑐𝑝 − 𝑐𝑣)𝑇𝑐𝑝
𝑐𝑣
The density in the nozzle is then calculated from conservation of mass flow. 
𝜌0𝜈outlet𝐴outlet = 𝑚̇ 
This  is  different  from  the  standard  LS-DYNA  jetting  formulation,  which  assumes  that 
the density of the gas in the jet is the same as atmospheric air, and then calculates the jet 
velocity from conservation of mass flow.
The  velocity  distribution  at  any  radius,  𝑟,  from  the  jet  centerline  and  distance,  𝑧,  from 
the focus,  𝑣𝑟,𝑧relates to the velocity of the jet centerline, 𝑣𝑟 = 0, 𝑧, in the same way as the 
standard LS-DYNA jetting options: 
𝑣𝑟,𝑧 = 𝑣𝑟=0,𝑧𝑒−( 𝑟
𝛼𝑧)
The  velocity  at  the  jet  centerline,  𝑣𝑟 = 0,  at  the  distance,  𝑧,  from  the  focus  of  the  jet  is 
calculated such that the momentum in the jet is conserved. 
momentum at nozzle = momentum at z 
𝜌0𝑣outlet
𝐴outlet = 𝜌0 ∫ 𝑣jet
2 𝑑𝐴jet 
= 𝜌0𝑣𝑟=0,𝑍
{𝑏 + 𝐹√𝑏} 
where, 𝑏 = 𝜋(𝛼𝑧)2
, and 𝐹 is the distance between the jet foci (for a passenger jet). 
Finally, the pressure exerted on an airbag element in view of the jet is given as: 
By combining the equations above 
2  
𝑝𝑟,𝑧 = 𝛽𝜌0𝑣𝑟,𝑧
𝑝𝑟,𝑧 =
]
𝛽𝑚̇ 𝑣outlet[𝑒−(𝑟/𝛼𝑧)2
{⎧𝜋(𝛼𝑧)2
⎩{⎨
+ 𝐹√𝜋(𝛼𝑧)2
}⎫
⎭}⎬
The total force exerted by the jet is given by 
𝐹jet = 𝑚̇ 𝑣outlet, 
which  is  independent  of  the  distance  from  the  nozzle.    Mass  flow  in  the  jet  is  not 
necessarily  conserved,  because  gas  is  entrained  into  the  jet  from  the  surrounding 
volume.    By  contrast,  the  standard  LS-DYNA  jetting  formulation  conserves  mass  flow 
but  not  momentum.    This  has  the  effect  of  making  the  jet  force  reduce  with  distance 
from the nozzle. 
The  jetting  forces  can  be  reacted  onto  a  node  (NREACT),  to  allow  the  reaction  force 
through the steering column or the support brackets to be modeled.  The jetting force is 
written to the ASCII abstat file and the binary xtf file.
*AIRBAG 
Additional  card  required  for  LOAD_CURVE  option.    (For  card  1  see  the  “core  cards” 
section of *AIRBAG.) 
  Card 2 
1 
2 
Variable 
STIME 
LCID 
Type 
F 
I 
3 
RO 
F 
4 
PE 
F 
5 
P0 
F 
6 
T 
F 
7 
T0 
F 
8 
Default 
0.0 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
Time at which pressure is applied.  The load curve is offset by this
amount. 
Load  curve  ID  defining  pressure  versus  time,  see  *DEFINE_-
CURVE. 
Initial density of gas (ignored if LCID > 0) 
Ambient pressure (ignored if LCID > 0) 
Initial gauge pressure (ignored if LCID > 0) 
Gas Temperature (ignored if LCID > 0) 
Absolute zero on temperature scale (ignored if LCID > 0) 
STIME 
LCID 
RO 
PE 
P0 
T 
T0 
Remarks: 
Within  this  simple  model  the  control  volume  is  inflated  with  a  pressure  defined  as  a 
function of time or calculated using the following equation if LCID = 0. 
𝑃total = 𝐶𝜌(𝑇 − 𝑇0) 
𝑃gauge = 𝑃total − 𝑃ambient 
The pressure is uniform throughout the control volume.
*AIRBAG_LINEAR_FLUID 
Additional card required for LINEAR_FLUID option.  (For card 1 see the “core cards” 
section of *AIRBAG.) 
  Card 2 
1 
Variable 
BULK 
Type 
F 
2 
RO 
F 
3 
4 
5 
6 
7 
8 
LCINT 
LCOUTT 
LCOUTP 
LCFIT 
LCBULK 
LCID 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none  optional optional optional  optional 
none 
Card 3 is optional.  
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
P_LIMIT  P_LIMLC 
Type 
F 
I 
Default  optional  optional 
  VARIABLE   
BULK 
DESCRIPTION
K, bulk modulus of the fluid in the control volume.  Constant as a
function of time.  Define if LCBULK = 0. 
RO 
𝜌, density of the fluid 
LCINT 
LCOUTT 
LCOUTP 
LFIT 
𝐹(𝑡) input flow curve defining mass per unit time as a function of
time, see *DEFINE_CURVE. 
𝐺(𝑡), output flow curve defining mass per unit time as a function
of time.  This load curve is optional.
𝐻(𝑝), output flow curve defining mass per unit time as a function
of pressure.  This load curve is optional.
𝐿(𝑡),  added  pressure  as  a  function  of  time.    This  load  curve  is 
optional.
VARIABLE   
LCBULK 
DESCRIPTION
Curve defining the bulk modulus as a function of time.  This load
curve is optional, but if defined, the constant, BULK, is not used.
LCID 
Load  curve  ID  defining  pressure  versus  time,  see  *DEFINE_-
CURVE. 
P_LIMIT 
Limiting value on total pressure (optional). 
P_LIMLC 
Curve defining the limiting pressure value as a function of time.
If nonzero, P_LIMIT is ignored. 
Remarks: 
If LCID = 0 then the pressure is determined from: 
𝑃(𝑡) = 𝐾(𝑡)ln [
𝑉0(𝑡)
𝑉(𝑡)
] + 𝐿(𝑡). 
where, 
𝑃(𝑡) = Pressure, 
𝑉(𝑡) = Volume of fluid in compressed state, 
𝑉0(𝑡) = 𝑉0(𝑡) 
=
𝑀(𝑡)
= Volume of fluid in uncompressed state, 
𝑀(𝑡) = 𝑀(0) + ∫ 𝐹(𝑡)𝑑𝑡 − ∫ 𝐺(𝑡)𝑑𝑡 − ∫ 𝐻(𝑝)𝑑𝑡 
= Current fluid mass, 
𝑀(0) = 𝑉(0)𝜌 
= Mass of fluid at time zero 𝑃(0) = 0. 
By setting LCID ≠ 0 a pressure time history may be specified for the control volume and 
the mass of fluid within the volume is then calculated from the volume and density. 
This  model  is  for  the  simulation  of  hydroforming  processes  or  similar  problems.    The 
pressure is controlled by the mass flowing into the volume and by the current volume.  
The pressure is uniformly applied to the control volume.   
Note the signs used in the equation for 𝑀(𝑡).  The mass flow should always be defined 
as positive since the output flow is subtracted.
*AIRBAG_HYBRID_OPTIONS 
*AIRBAG_HYBRID_JETTING_OPTIONS 
Additional cards required for HYBRID and HYBRID_JETTING options.  (For card 1 see 
the “core cards” section of *AIRBAG.) 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ATMOST  ATMOSP  ATMOSD 
GC 
CC 
HCONV 
Type 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
1.0 
none 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
C23 
LCC23 
A23 
LCA23 
CP23 
LCP23 
AP23 
LCAP23 
Type 
F 
Default 
none 
  Card 4 
1 
I 
0 
2 
F 
none 
3 
I 
0 
4 
F 
none 
5 
I 
0 
6 
F 
none 
7 
I 
0 
8 
Variable 
OPT 
PVENT 
NGAS 
LCEFR 
LCIDM0 
VNTOPT 
Type 
I 
F 
I 
Default 
none 
none 
none 
I 
0 
I 
0 
I
Include NGAS pairs of cards 5 and 6: 
  Card 5 
1 
2 
3 
4 
5 
Variable 
LCIDM 
LCIDT 
MW 
INITM 
Type 
I 
I 
F 
F 
6 
A 
F 
7 
B 
F 
8 
C 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FMASS 
Type 
F 
Default 
none 
  VARIABLE   
DESCRIPTION
ATMOST 
Atmospheric temperature 
ATMOSP 
Atmospheric pressure 
ATMOSD 
Atmospheric density 
GC 
CC 
HCONV 
Universal molar gas constant 
Conversion constant 
EQ.0: Set to 1.0. 
Effective  heat  transfer  coefficient  between  the  gas  in  the  air  bag
and the environment at temperature at ATMOST.  If HCONV < 0, 
then HCONV defines a load curve of data pairs (time, hconv). 
C23 
Vent  orifice  coefficient  which  applies  to  exit  hole.    Set  to  zero  if
LCC23 is defined below.
LCC23 
A23 
LCA23 
CP23 
LCCP23 
*AIRBAG_HYBRID 
DESCRIPTION
The  absolute  value,  |LCC23|,  is  a  load  curve  ID.    If  the  ID  is 
positive, the load curve defines the vent orifice coefficient which 
applies to exit hole as a function of time.  If the ID is negative, the
vent  orifice  coefficient  is  defined  as  a  function  of  relative
pressure, 𝑃air/𝑃bag, see [Anagonye and Wang 1999].  In addition,
LCC23  can  be  defined  through  *DEFINE_CURVE_FUNCTION. 
A nonzero value for C23 overrides LCC23  
If defined as a positive number, A23 is the vent orifice area which
applies to exit hole.  If defined as a negative number, the absolute
value |A23| is a part ID, see [Anagonye and Wang 1999].  The area
of  this  part  becomes  the  vent  orifice  area.    Airbag  pressure  will
not  be  applied  to  part  |A23|  representing  venting  holes  if  part 
|A23| is not included in SID, the part set representing the airbag.
Set A23 to zero if LCA23 is defined below. 
Load  curve  number  defining  the  vent  orifice  area  which  applies
to  exit  hole  as  a  function  of  absolute  pressure,  or  LCA23  can  be 
defined  through  *DEFINE_CURVE_FUNCTION.    A  nonzero 
value for A23 overrides LCA23. 
Orifice  coefficient  for  leakage  (fabric  porosity).    Set  to  zero  if
LCCP23 is defined below. 
Load  curve  number  defining  the  orifice  coefficient  for  leakage
(fabric porosity) as a function of time, or LCCP23 can be defined 
through  *DEFINE_CURVE_FUNCTION.    A  nonzero  value  for 
CP23 overrides LCCP23. 
AP23 
Area for leakage (fabric porosity) 
LCAP23 
Load curve number defining the area for leakage (fabric porosity)
as  a  function  of  (absolute)  pressure,  or  LCAP23  can  be  defined
through  *DEFINE_CURVE_FUNCTION.    A  nonzero  value  for 
AP23 overrides LCAP23.
VARIABLE   
OPT 
DESCRIPTION
Fabric  venting  option,  if  nonzero  CP23,  LCCP23,  AP23,  and
LCAP23 are set to zero. 
EQ.1: Wang-Nefske formulas for venting through an orifice are
used.  Blockage is not considered. 
EQ.2: Wang-Nefske formulas for venting through an orifice are
used.  Blockage of venting area due to contact is consid-
ered. 
EQ.3: Leakage  formulas  of  Graefe,  Krummheuer,  and  Siejak
[1990] are used.  Blockage is not considered. 
EQ.4: Leakage  formulas  of  Graefe,  Krummheuer,  and  Siejak 
[1990] are used.  Blockage of venting area due to contact
is considered. 
EQ.5: Leakage formulas based on flow through a porous media
are used.  Blockage due to contact is not considered.   
EQ.6: Leakage formulas based on flow through a porous media 
are used.  Blockage due to contact is considered.   
EQ.7: Leakage is based on gas volume outflow versus pressure
load  curve.    Blockage  of  flow  area  due  to  contact  is  not
considered.    Absolute  pressure  is  used  in  the  porous-
velocity-versus-pressure  load  curve, given  as FAC(𝑃)  in 
the *MAT_FABRIC card. 
EQ.8: Leakage is based on gas volume outflow versus pressure
load curve.  Blockage of flow area due to contact is con-
sidered. 
PVENT 
Gauge pressure when venting begins 
NGAS 
LCEFR 
LCIDM0 
Number of gas inputs to be defined below (Including initial air).
The maximum number of gases is 17. 
Optional  curve  for  exit  flow  rate  (mass/time)  versus  (gauge)
pressure 
Optional  curve  representing  inflator’s  total  mass  inflow  rate.
When  defined,  LCIDM  in  the  following  2 × NGAS  cards  defines 
the  molar  fraction  of  each  gas  component  as  a  function  of  time
and INITM defines the initial molar ratio of each gas component.
*AIRBAG_HYBRID 
DESCRIPTION
VNTOPT 
Additional options for venting area definition. 
For A23 ≥ 0 
EQ.1:  Vent area is equal to A23. 
EQ.2:  Vent  area  is  A23  plus  the  eroded  surface  area  of  the
airbag parts. 
EQ.10:  Same as VNTOPT = 2 
For A23 < 0 
EQ.1:  Vent area is the increase in surface area of part |A23|.   If 
there is no change in surface area of part |A23| over the 
initial  surface  area  or  if  the  surface  area  reduces  from
the initial area, there is no venting. 
EQ.2:  Vent area is the total (not change in) surface area of part
|A23|  plus  the  eroded  surface  area  of  all  other  parts
comprising the airbag. 
EQ.10:  Vent  area  is  the  increase  in  surface  area  of  part  |A23|
plus the eroded surface area of all other parts compris-
ing the airbag. 
LCIDM 
Load curve ID for inflator mass flow rate (eq.  0 for gas in the bag
at time = 0) 
GT.0: piecewise linear interpolation 
LT.0:  cubic spline interpolation 
LCIDT 
Load curve ID for inflator gas temperature (eq.0 for gas in the bag
at time 0) 
GT.0: piecewise linear interpolation 
LT.0:  cubic spline interpolation 
MW 
Molecular weight 
INITM 
Initial mass fraction of gas component present in the airbag, prior 
to injection of gas by the inflator 
A 
B 
Coefficient  for  molar  heat  capacity  of  inflator  gas  at  constant
pressure, (e.g., Joules/mole/oK) 
Coefficient  for  molar  heat  capacity  of  inflator  gas  at  constant
pressure, (e.g., Joules/mole/oK2)
VARIABLE   
DESCRIPTION
C 
Coefficient  for  molar  heat  capacity  of  inflator  gas  at  constant
pressure, (e.g., Joules/mole/oK3) 
FMASS 
Fraction of additional aspirated mass. 
Aditional cards are required for HYBRID_JETTING and HYBRID_JETTING_CM 
The following two additional cards are defined for the HYBRID_JETTING options.  The 
jet may be defined by specifying either the coordinates of the jet focal point, jet vector 
head  and  secondary  jet  focal  point,  or  by  specifying  three  nodes  located  at  these 
positions.    The  nodal  point  option  is  recommended  when  the  location  of  the  airbag 
changes as a function of time. 
  Card 7 
1 
2 
3 
4 
5 
6 
Variable 
XJFP 
YJFP 
ZJFP 
XJVH 
YJVH 
ZJVH 
Type 
F 
F 
F 
F 
F 
F 
7 
CA 
F 
8 
BETA 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Remark 
1 
  Card 8 
1 
1 
2 
1 
3 
1 
4 
1 
5 
1 
6 
7 
8 
Variable 
XSJFP 
YSJFP 
ZSJFP 
PSID 
IDUM 
NODE1 
NODE2 
NODE3 
Type 
F 
F 
F 
I 
F 
Default 
none 
none 
none 
none 
none 
Remark 
2 
I 
0 
1 
I 
0 
1 
I 
0
Additional card required for HYBRID_JETTING_CM option. 
  Card 9 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NREACT 
Type 
I 
Default 
none 
Remark 
4 
  VARIABLE   
DESCRIPTION
XJFP 
YJFP 
ZJFP 
XJVH 
YJVH 
ZJVH 
CA 
𝑥-coordinate of jet focal point, i.e., the virtual origin in Figures 3-1
and 3-2.  See Remark 1 below. 
𝑦-coordinate of jet focal point, i.e., the virtual origin in Figures 3-1
and 3-2. 
𝑧-coordinate of jet focal point, i.e., the virtual origin in Figures 3-1
and 3-2. 
𝑥-coordinate of jet vector head to defined code centerline 
𝑦-coordinate of jet vector head to defined code centerline 
𝑧-coordinate of jet vector head to defined code centerline 
Cone angle, 𝛼, defined in radians. 
LT.0.0: |𝛼| is the load curve ID defining cone angle as a function
of time 
BETA 
Efficiency  factor,  𝛽,  which  scales  the  final  value  of  pressure 
obtained from Bernoulli’s equation. 
LT.0.0: ∣𝛽∣ is the load curve ID defining the efficiency factor as a
function of time 
XSJFP 
𝑥-coordinate  of  secondary  jet  focal  point,  passenger  side  bag.    If
the  coordinate  of  the  secondary  point  is  (0,0,0)  then  a  conical  jet 
(driver’s side airbag) is assumed. 
YSJFP 
𝑦-coordinate of secondary jet focal point
VARIABLE   
DESCRIPTION
ZSJFP 
PSID 
𝑧-coordinate of secondary jet focal point 
Optional  part  set  ID,  see  *SET_PART.    If  zero  all  elements  are 
included in the airbag. 
IDUM 
Dummy field (Variable not used) 
NODE1 
Node  ID  located  at  the  jet  focal  point,  i.e.,  the  virtual  origin  in
Figure 3-7.  See Remark 1 below. 
NODE2 
Node ID for node along the axis of the jet. 
NODE3 
Optional node ID located at secondary jet focal point. 
NREACT 
Node  for  reacting  jet  force.    If  zero  the  jet  force  will  not  be
applied. 
Remarks: 
1.  Jetting.  It is assumed that the jet direction is defined by the coordinate method 
(XJFP, YJFP, ZJFP) and (XJVH, YJVH, ZJVH) unless both NODE1 and NODE2 
are  defined.    In  which  case  the  coordinates  of  the  nodes  given  by  NODE1, 
and 
NODE2 
(XJVH, YJVH, ZJVH).  The use of nodes is recommended if the airbag system is 
undergoing rigid body motion.  The nodes should be attached to the vehicle to 
allow for the coordinates of the jet to be continuously updated with the motion 
of the vehicle. 
and  NODE3  will 
(XJFP, YJFP, ZJFP) 
override 
The jetting option provides a simple model to simulate the real pressure distri-
bution in the airbag during the breakout and early unfolding phase.  Only the 
surfaces that are in the line of sight to the virtual origin have an increased pres-
sure  applied.    With  the  optional  load  curve  LCRJV,  the  pressure  distribution 
with the code can be scaled according to the so-called relative jet velocity distri-
bution.   
For  passenger  side  airbags  the  cone  is  replaced  by  a  wedge  type  shape.    The 
first  and  secondary  jet  focal  points  define  the  corners  of  the  wedge  and  the 
angle 𝛼 then defines the wedge angle. 
Instead  of  applying  pressure  to  all  surfaces  in  the  line  of  sight  of  the  virtual 
origin(s), a part set can be defined to which the pressure is applied. 
2. 
IDUM.    This  variable  is  not  used  and  has  been  included  to  maintain  the  same 
format as the WANG_NEFSKE_JETTING options.
3.  Focal Point Placement.  Care must be used to place the jet focal point within 
the bag.  If the focal point is outside the bag, inside surfaces will not be visible 
so jetting pressure will not be applied correctly. 
4.  NREACT.    See  the  description  related  to  the  WANG_NEFSKE_JETTING_CM 
option.  For the hybrid inflator model the heat capacities are compute from the 
combination of gases which inflate the bag.
*AIRBAG_HYBRID_CHEMKIN_OPTION 
The  HYBRID_CHEMKIN  model  includes  3  control  cards.    For  each  gas  species  an 
additional  set  of  cards  must  follow  consisting  of  a  control  card  and  several 
thermodynamic  property  data  cards.    (For  card  1  see  the  “core  cards”  section  of 
*AIRBAG.) 
  Card 2 
1 
2 
3 
4 
5 
6 
Variable 
LCIDM 
LCIDT 
NGAS 
DATA 
ATMT 
ATMP 
Type 
I 
I 
I 
I 
F 
F 
8 
7 
RG 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
HCONV 
Type 
F 
Default 
0. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
C23 
A23 
Type 
F 
Default 
0. 
F 
0. 
  VARIABLE   
DESCRIPTION
LCIDM 
Load curve specifying input mass flow rate versus time. 
GT.0: piece wise linear interpolation 
LT.0:  cubic spline interpolation
*AIRBAG_HYBRID_CHEMKIN 
DESCRIPTION
LCIDT 
Load curve specifying input gas temperature versus time. 
GT.0: piece wise linear interpolation 
LT.0:  cubic spline interpolation 
NGAS 
DATA 
Number of gas inputs to be defined below.  (Including initial air) 
Thermodynamic database 
EQ.1: NIST database (3 additional property cards are required
below) 
EQ.2: CHEMKIN  database  (no  additional  property  cards  are 
required) 
EQ.3: Polynomial  data  (1  additional  property  card  is  required
below) 
ATMT 
ATMP 
Atmospheric temperature. 
Atmospheric pressure 
RG 
Universal gas constant 
HCONV 
Effective  heat  transfer  coefficient  between  the  gas  in  the  air  bag 
and the environment at temperature ATMT.  If HCONV < 0, then 
HCONV defines a load curve of data pairs (time, hconv). 
C23 
A23 
Vent orifice coefficient 
Vent orifice area
NGAS Sets of Gas Species Data Cards: 
For  each  gas  species  include  a  set  of  cards  consisting  of  a  Gas  Species  Control  Card 
followed by several thermo-dynamic property data cards whose format depends on the 
DATA parameter on card in format “card 5”.  The next "*" card terminates the reading 
of this data. 
Gas Species Control Card. 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CHNAME 
MW 
LCIDN 
FMOLE 
FMOLET 
Type 
A 
F 
Default 
none 
none 
I 
0 
F 
F 
none 
0. 
  VARIABLE   
CHNAME 
DESCRIPTION
Chemical symbol for this gas species (e.g., N2 for nitrogen, AR for 
argon). 
Required  for  DATA = 2  (CHEMKIN),  optional  for  DATA = 1  or 
DATA = 3. 
MW 
Molecular weight of this gas species. 
LCIDN 
Load curve specifying the input mole fraction versus time for this
gas species.  If > 0, FMOLE is not used. 
FMOLE 
Mole fraction of this gas species in the inlet stream. 
FMOLET 
Initial mole fraction of this gas species in the tank. 
Additional thermodynamic data cards for each gas species.
If DATA = 1, include the following 3 cards for the NIST database: 
The  required  data  can  be  found  on  the  NIST  web  site  at  http://webbook.nist.gov/
chemistry/. 
  Card 5a 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TLOW 
TMID 
THIGH 
Type 
F 
F 
F 
Default 
none 
none 
none 
  Card 5b 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
alow 
blow 
clow 
dlow 
elow 
flow 
hlow 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
  Card 5c 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ahigh 
bhigh 
chigh 
dhigh 
ehigh 
fhigh 
hhigh 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
TLOW 
TMID 
Curve fit low temperature limit. 
Curve fit low-to-high transition temperature. 
THIGH 
Curve fit high temperature limit.
VARIABLE   
alow, …, hlow 
DESCRIPTION
Low  temperature  range  NIST  polynomial  curve  fit  coefficients 
. 
ahigh, …, hhigh 
High  temperature  range  NIST  polynomial  curve  fit  coefficients
. 
No additional cards are needed if using the CHEMKIN database (DATA = 2): 
6 
7 
8 
Polynomial Fit Card (DATA = 3). 
  Card 5d 
Variable 
Type 
1 
a 
F 
2 
b 
F 
3 
c 
F 
4 
d 
F 
5 
e 
F 
Default 
none 
0. 
0. 
0. 
0. 
  VARIABLE   
DESCRIPTION
a 
b 
c 
d 
e 
Coefficient, see below. 
Coefficient, see below. 
Coefficient, see below. 
Coefficient, see below. 
Coefficient, see below. 
Specific heat curve fits: 
NIST:
𝑐𝑝 =
CHEMKIN:
𝑐𝑝 =
POLYNOMIAL:
𝑐𝑝 =
(𝑎 + 𝑏𝑇 + 𝑐𝑇2 + 𝑑𝑇3 +
𝑇2)
(𝑎 + 𝑏𝑇 + 𝑐𝑇2 + 𝑑𝑇3 + 𝑒𝑇4)
(𝑎 + 𝑏𝑇 + 𝑐𝑇2 + 𝑑𝑇3 + 𝑒𝑇4)
𝑅̅̅̅̅̅
𝑅̅̅̅̅̅ = universal gas constant 8.314
Nm
mole × 𝐾
where,
𝑀 = gas molecular weight
*AIRBAG_FLUID_AND_GAS_OPTIONS 
Additional  cards  required  for  FLUID_AND_GAS  option.    (For  card  1  see  the  “core 
cards”  section  of  *AIRBAG.)  Currently  this  option  only  works  in  SMP  and  explicit 
analysis. 
  Card 2 
1 
2 
3 
Variable 
XWINI 
XWADD 
XW 
Type 
F 
F 
F 
4 
P 
F 
5 
6 
7 
8 
TEND 
RHO 
LCXW 
LCP 
F 
F 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
GDIR 
NPROJ 
IDIR 
IIDIR 
KAPPA 
KBM 
Type 
F 
Default 
none 
I 
3 
I 
I 
F 
F 
none 
none 
1.0 
none 
  VARIABLE   
DESCRIPTION
XWINI 
Fluid level at time 𝑡 = 0 in |GDIR| direction. 
XWADD 
Fluid level filling increment per time step. 
XW 
P 
Final fluid level in filling process. 
Gas pressure at time 𝑡 = TEND.
TEND 
Time when gas pressure P is reached.
RHO 
LCXW 
LCP 
Density of the fluid (e.g.  for water, RHO ≈ 1.0 kg/m3) 
Load curve ID for fluid level vs.  time.  XW, XWADD, and XWINI
are with this option. 
Load  curve  ID  for  gas  pressure  vs.    time.    P  and  TEND  are
ignored with this option.
GDIR 
*AIRBAG_FLUID_AND_GAS 
DESCRIPTION
Global direction of gravity (e.g.  -3.0 for negative global z-axis).  
EQ.1.0: global 𝑥-direction, 
EQ.2.0: global 𝑦-direction, 
EQ.3.0: global 𝑧-direction. 
NPROJ 
IDIR 
IIDIR 
Number  of  projection  directions  (only  global  axis)  for  volume
calculation. 
First direction of projection (if ∣NPROJ∣ ≠ 3), only global axis. 
Second direction of projection (if |NPROJ| = 2), only global axis.
KAPPA 
Adiabatic exponent 
KBM 
Bulk modulus of the fluid (e.g.  for water, BKM ≈ 2080 N/mm2) 
Remarks: 
The  *AIRBAG_FLUID_AND_GAS  option  models  a  quasi-static  multi  chamber 
fluid/gas structure interaction in a simplified way including three possible load cases: 
(i)  only  gas,  (ii)  only  incompressible  fluid,  or  (iii)  the  combination  of  incompressible 
fluid with additional gas “above”.   see Figure 3-5. 
Figure 3-5.  Hydrostatic pressure distribution in a chamber filled with gas and
incompressible fluid 
The  theory  is  based  on  the  description  of  gases  and  fluids  as  energetically  equivalent 
pressure loads.  The calculation of the fluid volume is carried out using the directions of 
projection and a non-normalized normal vector.  This model, therefore, requires that the 
normal of the shell elements belonging to a filled structure must point outwards.  Holes 
are not detected, but can be taken into account as described below.
In  case  of  a  pure  gas  (no  fluid),  the  *AIRBAG_SIMPLE_PRESSURE_VOLUME  and 
*AIRBAG_FLUID_AND_GAS cards give identical results as they are based on the same 
theory.    The  update  of  the  gas  pressure  due  to  volume  change  is  calculated  with  the 
following simple gas law 
𝑝𝑔 =
⎜⎛1 − KAPPA ×
⎝
𝑣𝑔 − 𝑣old
𝑣old
𝑔  
⎟⎞ 𝑝old
⎠
with adiabatic exponent KAPPA and gas volume 𝑣𝑔. 
The theory of incompressible fluids is based on the variation of the potential energy and 
an  update  of  the  water  level  due  to  changes  in  the  volume  and  the  water  surface,  see 
Haßler  and  Schweizerhof  [2007],  Haßler  and  Schweizerhof  [2008],  Rumpel  and 
Schweizerhof [2003], and Rumpel and Schweizerhof [2004].  
In  case  of  multiple  fluid/gas  filled  chambers  each  chamber  requires  an  additional 
*AIRBAG_FLUID_AND_GAS  card.    Some  of  the  parameters  which  are  called  local 
parameters  only  belong  to  a  single  chamber  (e.g.    gas  pressure).    In  contrast  global, 
parameters belong to all chambers (e.g.  direction of gravitation). 
Because the theory only applies to quasi-static fluid-structure interaction the load has to 
be applied slowly so that the kinetic energy is almost zero throughout the process. 
All parameters of card 1 are local parameters describing the filling of the chamber.  The 
water  level  and  the  gas  pressure  can  be  defined  by  curves  using  LCXW  and  LCP.    A 
second  possibility  are  the  parameters  XWINI,  XW,  XWADD,  P  and  TEND.    When 
describing the fluid and gas filling using the parameters the gas pressure at time 𝑡 = 0 is 
set  to  0  and  the  initial  water  level  is  set  to  XWINI  in  |GDIR|-direction.    At  each 
timestep, XWADD is  added to the water level, until XW is reached.  The gas pressure 
will be raised until P is reached at time 𝑡 = TEND. 
In  general,  global  parameters  belong  to  all  chambers.    To  describe  the  global  axis  in 
GDIR,  NPROJ,  IDIR  and  IIDIR  the  following  relations  apply:  𝑥-axis  is  axis  “1”,  the  𝑦-
axis is axis “2”, and the 𝑧-axis is axis 3. 
The  gas  and  fluid  volume  is  calculated  by  contour  integrals  in  the  global  𝑥-,  𝑦-  and  𝑧-
coordinates.  If one of the boundaries is discontinuous in one or two global directions, 
these directions have to be ignored in NPROJ, IDIR and IIDIR.  At least one direction of 
projection must be set (NPROJ = 1, IDIR = value), but it is recommended to use as many 
directions of projection as possible.  
In case of a structure filled exclusively with fluid, IDIR and IIDIR should not be set to 
|GDIR|.    In  case  of  holes  in  a  structure  (e.g.    to  take  advantage  of  symmetry  planes), 
IDIR  and  IIDIR  should  not  be  set  to  the  normal  direction  of  the  plane  describing  the 
hole or symmetry plane.
An example of a water filled tube structure illustrating how to use NPROJ, IDIR, IIDIR, 
and  GDIR  is  shown  in  Figure  3-6.    In  this  example  gravity  is  acting  opposite  to  the 
global  𝑧-axis.    In  this  case,  then,  GDIR = -3.    The  structure  is  filled  exclusively  with 
water, so the projection direction cannot be set to |GDIR| = 3.  To use the symmetry of 
the  tube  only  half  of  the  structure  has  been  modeled.    The  normal  of  the  symmetry 
plane  shows  in  𝑦  direction,  so  the  projection direction  cannot  be  set  to  2.    Because  the 
symmetry axes (2 and 3) are not allowed, the only direction of projection is 1; therefore, 
NPROJ = 1 and IDIR = 1. 
Figure 3-6.  Example for water filled tube structure 
For further explanations and examples see Haßler and Schweizerhof [2007], Haßler and 
Schweizerhof [2008], and Maurer, Gebhardt, and Schweizerhof [2010]. 
The possible entries for NPROJ, IDIR and IIDIR are: 
NPROJ
IDIR IIDIR
3 
2 
2 
2 
1 
1 
1 
2 
3 
3 
1 
1 
2 
1 
2
*AIRBAG 
Purpose:    The  input  in  this  section  provides  a  simplified  approach  to  defining  the 
deployment of the airbag using the ALE capabilities with an option to switch from the 
initial  ALE  method  to  control  volume  (CV)  method  (*AIRBAG_HYBRID)  at  a  chosen 
time.    An  enclosed  airbag  (and  possibly  the  airbag  canister/compartment  and/or  a 
simple  representation  of  the  inflator)  shell  structure  interacts  with  the  inflator  gas(es).  
This  definition  provides  a  single  fluid  to  structure  coupling  for  the  airbag-gas 
interaction during deployment in which the CV input data may be used directly. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
SIDTYP 
MWD 
SPSF 
Type 
I 
I 
Default 
none 
none 
F 
0 
F 
0 
Remark 
1 
  VARIABLE   
SID 
DESCRIPTION
Set  ID  as  defined  on  *AIRBAG  card.    This  set  ID  contains  the
Lagrangian  elements  (segments)  which  make  up  the  airbag  and
possibly  the  airbag  canister/compartment  and/or  a  simple
representation of the inflator.  See Remark 1. 
SIDTYP 
Set type: 
EQ.0: Segment set. 
EQ.1: Part set. 
MWD 
SPSF 
Mass  weighted  damping  factor,  D.    This  is  used  during  the  CV
phase for *AIRBAG_HYBRID. 
Stagnation  pressure  scale  factor,  0 ≤ 𝛾 ≤ 1.    This  is  used  during 
the CV phase for *AIRBAG_HYBRID.
Card 2 
1 
2 
3 
Variable 
ATMOST  ATMOSP 
Type 
F 
Default 
0. 
Remark 
2 
F 
0. 
2 
*AIRBAG_ALE 
4 
GC 
F 
5 
6 
7 
8 
CC 
TNKVOL 
TNKFINP 
F 
F 
F 
none 
1.0 
0.0 
0.0 
10 
10 
  VARIABLE   
DESCRIPTION
ATMOST 
Atmospheric ambient temperature.  See Remark 2. 
ATMOSP 
Atmospheric ambient pressure.  See Remark 2. 
GC 
CC 
TNKVOL 
Universal molar gas constant. 
Conversion constant.  If EQ: .0 Set to 1.0. 
Tank  volume  from  the  inflator  tank  test  or  Inflator  canister
volume.  See remark 10. 
LCVEL = 0 and TNKFINP is defined: 
TNKVOL is the defined Tank.  Inlet gas velocity is estimat-
ed by LS-DYNA method (testing). 
LCVEL = 0 and TNKFINP is not defined 
TNKVOL  is  the  estimated  inflator  canister  volume  Inlet
gas  velocity  is  estimated  automatically  by  the  Lian-
Bhalsod-Olovsson  method. 
LCVEL ≠ 0 
This must be left blank. 
TNKFINP 
Tank final pressure from the inflator tank test data.  Only define
this  parameter  for  option  1  of  TNKVOL  definition  above.    See
Remark 10.
Coupling Card.  See keyword *CONSTRAINED_LAGRANGE_IN_SOLID.  
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NQUAD 
CTYPE 
PFAC 
FRIC 
FRCMIN  NORMTYP 
ILEAK 
PLEAK 
Type 
Default 
I 
4 
I 
4 
F 
F 
F 
0.1 
0.0 
0.3 
I 
0 
I 
2 
F 
0.1 
Remark 
13 
13 
14 
  VARIABLE   
NQUAD 
DESCRIPTION
Number of (quadrature) coupling points for coupling Lagrangian
slave  parts  to  ALE  master  solid  parts.    If  NQUAD = n,  then  nXn 
coupling  points  will  be  parametrically  distributed  over  the
surface  of  each  Lagrangian  slave  segment  (default = 4).    See 
Remark 13. 
CTYPE 
Coupling type (default = 4, see Remark 13): 
PFAC 
EQ.4: (default) penalty coupling with DIREC = 2 implied. 
EQ.6: penalty coupling in which DIREC is automatically set to
DIREC = 1  for  the  unfolded  region  and  DIREC = 2  for 
folded region. 
Penalty  factor.    PFAC  is  a  scale  factor  for  scaling  the  estimated
stiffness  of  the  interacting  (coupling)  system.    It  is  used  to
compute  the  coupling  forces  to  be  distributed  on  the  slave  and
master parts. 
GT.0: Fraction of estimated critical stiffness (default = 0.1). 
LT.0:  -PFAC is a load curve ID.  The curve defines the relative
coupling  pressure  (y-axis)  as  a  function  of  the  tolerable 
fluid penetration distance (x-axis). 
FRIC 
Coupling coefficient of friction. 
FRCMIN 
Minimum  fluid  volume  fraction  in  an  ALE  element  to  activate 
coupling (default is 0.3).
*AIRBAG_ALE 
DESCRIPTION
NORMTYP 
Penalty coupling spring direction (DIREC 1 and 2): 
EQ.0: normal  vectors  are  interpolated  from  nodal  normals
(default) 
EQ.1: normal vectors are interpolated from segment normals. 
ILEAK 
Leakage control flag.  Default = 2 (with energy compensation). 
PLEAK 
Leakage control penalty factor (default = 0.1) 
Venting Hole Card. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IVSETID 
IVTYPE 
IBLOCK 
VNTCOF 
Type 
Default 
Remark 
I 
0 
4 
I 
0 
I 
0 
5 
F 
0.0 
6 
  VARIABLE   
DESCRIPTION
IVSETID 
Set ID defining the venting hole surface(s).  See Remark 4. 
IVTYPE 
Set type of IVSETID: 
EQ.0: Part Set (default). 
EQ.1: Part ID. 
EQ.2: Segment Set. 
IBLOCK 
Flag  for  considering  blockage  effects  for  porosity  and  vents  : 
EQ.0: no (blockage is NOT considered, default). 
EQ.1: yes (blockage is considered). 
VNTCOF 
Vent Coefficient for scaling the flow.  See Remark 6.
transformation. 
  Parameters  for  ALE  mesh  automatic  definition  and 
its 
*AIRBAG 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NX/IDA 
NY/IDG 
NZ 
MOVERN 
ZOOM 
Type 
I 
I 
I 
Default 
none 
none 
none 
Remark 
7 
7 
7 
I 
0 
8 
I 
0 
9 
  VARIABLE   
DESCRIPTION
Option 1: Automatic ALE mesh, activated by NZ.NE.0 (blank): 
NX 
NY 
NZ 
NX  is  the  number  of  ALE  elements  to  be  generated  in  the  x
direction.  See remark 7. 
NY  is  the  number  of  ALE  elements  to  be  generated  in  the  y
direction.  See remark 7. 
NZ  is  the  number  of  ALE  elements  to  be  generated  in  the  z
direction.  See remark 7. 
Option 2: ALE mesh from part ID: 
IDAIR 
IDAIR is the Part ID of the initial air mesh.  See remark 7. 
IDGAS 
IDGAS is defined as Part ID of the initial gas mesh.  See remark 7.
NZ 
Leave blank to activate options 2.  See remark 7. 
Variables common to both options: 
MOVERN 
ALE mesh automatic motion option . 
EQ.0: ALE mesh is fixed in space. 
GT.0:  Node  group  id.    See  *ALE_REFERENCE_SYSTEM_-
NODE  ALE  mesh  can  be  moved  with  PRTYP = 5,  mesh 
motion  follows  a  coordinate  system  defined  by  3  refer-
ence nodes.
*AIRBAG_ALE 
DESCRIPTION
ZOOM 
ALE mesh automatic expansion option : 
EQ.0: do not expand ALE mesh 
EQ.1: Expand/contract  ALE  mesh  by  keeping  all  airbag  parts
to
the  ALE  mesh 
(equivalent 
contained  within 
PRTYP = 9). 
Origin for ALE Mesh Card.  Include Cards 5a and 5b when NZ > 0. 
  Card 5a 
Variable 
1 
X0 
Type 
F 
2 
Y0 
F 
3 
Z0 
F 
4 
X1 
F 
5 
Y1 
F 
6 
Z1 
F 
7 
8 
Default 
none 
none 
none 
none 
none 
none 
  Card 5b 
Variable 
1 
X2 
Type 
F 
2 
Y2 
F 
3 
Z2 
F 
4 
Z3 
F 
5 
Y3 
F 
6 
Z3 
F 
7 
8 
Default 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
X0, Y0, Z0 
Coordinates of origin for ALE mesh generation (node0). 
X1, Y1, Z1 
Coordinates of point 1 for ALE mesh generation (node1). 
𝑥-extent = node1 − node0
X2, Y2, Z2 
Coordinates of point 2 for ALE mesh generation (node2). 
𝑦-extent = node2 − node0
X3, Y3, Z3 
Coordinates of point 3 for ALE mesh generation(node3). 
𝑧-extent = node3 − node0
(x4, y4, z4)
(x1, y1, z1)
(x2, y2, z2)
(
=
y(=3)
)
(x0, y0, z0)
8 )
x( =
Figure  3-7.   Illustration of automatic  mesh generation for the ALE mesh in a
hexahederal region 
Miscellaneous Parameters Card. 
3 
HG 
F 
0. 
4 
5 
6 
7 
8 
NAIR 
NGAS 
NORIF 
LCVEL 
LCT 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
10 
11 
  Card 6 
1 
2 
Variable 
SWTIME 
Type 
F 
Default 
1e16 
Remarks 
3 
  VARIABLE   
SWTIME 
DESCRIPTION
Time  to  switch  from  ALE  method  to  control  volume  (CV) 
method.    Once  switched,  a  method  similar  to  that  used  by  the
*AIRBAG_HYBRID card is used. 
HG 
NAIR 
Hourglass control for ALE fluid mesh(es). 
Number of Air components.  For example, this equals 2 in case air
contains 80% of N2 and 20% of O2.  If air is defined as 1 single gas
then NAIR = 1. 
NGAS 
Number of inflator Gas components.
NORIF 
LCVEL 
*AIRBAG_ALE 
DESCRIPTION
Number of point sources or orifices.  This determines the number 
of point source cards to be read. 
Load  curve  ID  for  inlet  velocity  .  This is the same estimated velocity curve used
in *SECTION_POINT_SOURCE_MIXTURE card. 
LCT 
Load curve ID for inlet gas temperature .
Air Component Card.  Include NAIR cards, one for each air component. 
  Card 7 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
Remarks 
MWAIR 
INITM 
AIRA 
AIRB 
AIRC 
F 
0 
F 
0 
F 
0 
F 
0. 
F 
0. 
12 
12 
12 
  VARIABLE   
DESCRIPTION
MWAIR 
Molecular weight of air component 
INITA 
AIRA 
AIRB 
AIRC 
Initial Mass Fraction of Air component(s) 
First Coefficient of molar heat capacity at constant pressure (e.g.,
J/mole/K, remark 12). 
Second  Coefficient  of  molar  heat  capacity  at  constant  pressure 
(e.g., J/mole/K2, remark 12). 
Third Coefficient of molar heat capacity at constant pressure (e.g.,
J/mole/K3, remark 12).
Gas Component Card.  Include NGAS cards, one for each gas component. 
  Card 8 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCMF 
MWGAS 
GASA 
GASB 
GASC 
Type 
I 
Default 
none 
F 
0 
F 
0 
F 
0. 
F 
0. 
Remarks 
11 
12 
12 
12 
  VARIABLE   
LCMF 
DESCRIPTION
Load  curve  ID  for  mass  flow  rate  . 
MWGAS 
Molecular weight of inflator gas components. 
GASA 
GASB 
GASC 
First Coefficient of molar heat capacity at constant pressure (e.g.,
J/mole/K, remark 12). 
Second  Coefficient  of  molar  heat  capacity  at  constant  pressure
(e.g., J/mole/K2, remark 12). 
Third Coefficient of molar heat capacity at constant pressure (e.g., 
J/mole/K3, remark 12). 
Point Source Cards.  Include NORIF cards, one for each point source. 
  Card 9 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NODEID 
VECID 
ORIFARE 
Type 
Default 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
NODEID 
The node ID defining the point source.
*AIRBAG_ALE 
DESCRIPTION
VECID 
The vector ID defining the direction of flow at the point source. 
ORIFARE 
The orifice area at the point source. 
Remarks: 
1.  This  set  ID  typically  contains  the  Lagrangian  segments  of  the  3  parts  that  are 
coupled to the inflator gas: airbag, airbag canister (compartment), inflator.  As 
in  all  control-volume,  orientation  of  elements  representing  bag  and  canister 
should  point  outward.    During  the  ALE  phase  the  segment  normal  will  be  re-
versed  automatically  for  fluid-structure  coupling.    However,  the  orientation  of 
inflator element normal vectors should point to its center.  See Figure 3-8. 
Bag fabric
Inflator
Canister
Figure 3-8.  Arrows indicate “outward” normal 
2.  Atmospheric density for the ambient gas (air) can be computed from 
𝜌amb =
𝑃amb
𝑅𝑇amb
3.  Since  ALL  ALE  related  activities  will  be  turned  off  after  the  switch  from  ALE 
method  to  control-volume  method,  no  other  ALE  coupling  will  exist  beyond 
t = SWTIME. 
4.  Vent  definition  will  be  used  for  ALE  venting.    Upon  switching  area  of  the 
segments will be used for venting as a23 in *AIRBAG_HYBRID.
5.  Fabric porosity for ALE and *AIRBAG_HYBRID can be defined on MAT_FAB-
RIC.  Define FLC and FAC on *MAT_FABRIC.  FVOPT 7 and 8 will be used for 
both  ALE  and  *AIRBAG_HYBRID.    IBLOCK = 0  will  use  FVOPT = 7  and 
IBLOCK = 1 will use FVOPT = 8.  
6.  VCOF  will  be  used  to  scale  the  vent  area  for  ALE  venting  and  this  coefficient 
will be used as vent coefficient c23 for *AIRBAG_HYBRID upon switching. 
7. 
8. 
If NX, NY and NZ are defined (option 1), card 5a and card 5b should be defined 
to let LS-DYNA generate the mesh for ALE.  Alternatively if NZ is 0 (option 2), 
then NX = IDAIR and NY = IDGAS.  In the latter case the user need to supply 
the ALE mesh whose PID = IDAIR. 
If the airbag moves with the vehicle, set MOVERN = GROUPID, this GROUPID 
is defined using *ALE_REFERENCE_SYSTEM_NODE.   The 3 nodes defined in 
ALE_REFERENCE_SYSTEM_NODE  will  be  used  to  transform  the  ALE  mesh.  
The point sources will also follow this motion.  This simulates PRTYP = 5 in the 
*ALE_REFERENCE_SYSTEM_GROUP card. 
9.  Automatic  expansion/contraction  of  the  ALE  mesh  to  follow  the  airbag 
expansion  can  be  turned  on  by  setting  zoom = 1.      This  feature  is  particularly 
useful  for  fully  folded  airbags  requiring  very  fine  ale  mesh  initially.    As  the 
airbag  inflates  the  ale  mesh  will  be  automatically  scaled  such  that  the  airbag 
will  be  contained  within  the  ALE  mesh.    This  simulates  PRTYP = 9  in  the 
*ALE_REFERENCE_SYSTEM_GROUP card. 
10.  There are 3 methods for defining the inlet gas velocity: 
a)  Inlet gas velocity is estimated by LSDYNA method (testing), if 
LCVEL = 0 ⇒ TNKVOL = Tank volume 
and 
TNKFINP = Tank final pressure from tank test data. 
b)  Inlet  gas  velocity  is  estimated  automatically  by  Lian-Bhalsod-Olovsson 
method if,  
LCVEL = 0 ⇒ TNKVOL = Tank volume. 
and 
TNKFINP = blank. 
c)  Inlet gas velocity is defined by user via a load curve LCVEL if, 
LCVEL  =  n, 
TNKVOL  = 0, 
and
11.  LCT and LCIDM should have the same number of sampling points. 
TNKFINP = 0 
12.  The per-mass-unit, temperature-dependent, constant-pressure heat capacity is 
𝐶𝑝(𝑇) =
[𝐴 + 𝐵𝑇 + 𝐶𝑇2]
𝑀𝑊
. 
where, 
these quantities often have units of, 
𝐴 = 𝐶̃𝑝0 
𝐶𝑝(𝑇) 
kg × K
𝐶 
mole × K
mole × K2
mole × K3 
13.  Sometimes  CTYPE = 6  may  be  used  for  complex  folded  airbag.    NQUAD = 2 
may  be  used  as  a  starting  value  and  increase  as  necessary  depending  on  the 
relative mesh resolutions of the Lagrangian and ALE meshes. 
14.  Use a load curve for PFAC whenever possible.  It tends to be more robust. 
Related Cards: 
AIR ⟶ 
GAS ⟶ 
{⎧*PART (AMMG2)
*SECTION_SOLID
⎩{⎨
*MAT_GAS_MIXTURE
{⎧*PART (AMMG1)
*SECTION_POINT_SOURCE_MIXTURE
⎩{⎨
*MAT_GAS_MIXTURE
Couplings ⟶  *CONSTRAINED_LAGRANGE_IN_SOLID 
ALE Mesh Motion ⟶  *ALE_REFERENCE_SYSTEM_GROUP 
Control Volume ⟶  *AIRBAG_HYBRID 
Vent ⟶  *AIRBAG_ALE/Card4 
Example 1: 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
*AIRBAG_ALE 
$#1    SID   SIDTYPE      NONE      NONE      NONE      NONE       MWD      SPSF 
       123         1         0         0         0         0       0.0       0.0
$#2 ATMOST    ATMOSP      NONE        GC        CC    TNKVOL     TNKFP 
    298.15 1.0132E-4         0     8.314       0.0       0.0       0.0 
$#3  NQUAD     CTYPE      PFAC      FRIC    FRCMIN  NRMTYPE     ILEAK     PLEAK 
         4         4     -1000       0.0       0.3         0         2       0.1 
$#4 VSETID  IVSETTYP    IBLOCK  VENTCOEF 
         1         2         0      1.00 
$#5NXIDAIR   NYIDGAS        NZ    MOVERN      ZOOM 
     50000     50003         0         0         0 
$#6 SWTIME      NONE        HG      NAIR      NGAS     NORIF     LCVEL       LCT 
   1000.00     0.000     1.e-4         1         1         8      2002      2001 
$#7 AIR         NONE      NONE     MWAIR     INITM      AIRA      AIRB      AIRC 
         0         0         0   0.02897      1.00    29.100   0.00000   0.00000 
$#8 GASLCM      NONE      NONE     MWGAS      NONE      GASA      GASB      GASC 
      2003         0         0    0.0235         0    28.000   0.00000   0.00000 
$#9 NODEID    VECTID  ORIFAREA 
    100019         1 13.500000 
    100020         2 13.500000 
    100021         3 13.500000 
    100022         4 13.500000 
    100023         5 13.500000 
    100024         6 13.500000 
    100017         7 13.500000 
    100018         8 13.500000 
$ PFAC CURVE = penalty factor curve. 
*DEFINE_CURVE 
$     lcid      sidr       sfa       sfo      offa      offo    dattyp 
      1000         0       0.0       2.0       0.0       0.0 
$                 a1                  o1 
                 0.0          0.00000000 
           1.0000000        4.013000e-04 
*SET_SEGMENT_TITLE 
vent segments (defined in IVSETID) 
         1       0.0       0.0       0.0       0.0 
      1735      1736       661      1697       0.0       0.0       0.0       0.0 
      1735      2337      1993      1736       0.0       0.0       0.0       0.0 
      1735      1969      1988      2337       0.0       0.0       0.0       0.0 
      1735      1697       656      1969       0.0       0.0       0.0       0.0 
*DEFINE_VECTOR 
$#     vid        xt        yt        zt        xh        yh        zh 
         1       0.0       0.0-16.250000 21.213200 21.213200-16.250000 
         2       0.0       0.0-16.250000 30.000000-1.000e-06-16.250000 
         3       0.0       0.0-16.250000 21.213200-21.213200-16.250000 
         4       0.0       0.0-16.250000-1.000e-06-30.000000-16.250000 
         5       0.0       0.0-16.250000-21.213200-21.213200-16.250000 
         6       0.0       0.0-16.250000-30.0000001.0000e-06-16.250000 
         7       0.0       0.0-16.250000-21.213200 21.213200-16.250000 
         8       0.0       0.0-16.2500001.0000e-06 30.000000-16.250000 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
In  this  example,  pre-existing  background  air  mesh  with  part  ID  50000  and  gas  mesh 
with  part  ID  50003  are  used.    Thus  NZ = 0.    There  is  no  mesh  motion  nor  expansion 
allowed.  An inlet gas velocity curve is provided. 
Example 2: 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
$ SIDTYP: 0=SGSID; 1=PSID 
*AIRBAG_ALE 
$#1    SID   SIDTYPE      NONE      NONE      NONE      NONE       MWD      SPSF 
         1         1         0        0.        0.        0.        0.        0. 
$#2 ATMOST    ATMOSP      NONE        GC        CC    TNKVOL     TNKFP 
      298.   101325.       0.0     8.314        1.    6.0E-5         0
$#3  NQUAD     CTYPE      PFAC      FRIC    FRCMIN  NRMTYPE     ILEAK     PLEAK 
         2         6      -321       0.0       0.3         1         2       0.1 
$#4 VSETID  IVSETTYP    IBLOCK  VENTCOEF 
         0         0         0         0   
$#5NXIDAIR   NYIDGAS        NZ    MOVERN      ZOOM 
        11        11         9   
$5b     x0        y0        z0        x1        y1        z1  NOT-USED  NOT-USED 
      -0.3      -0.3    -0.135       0.3      -0.3    -0.135 
$5c     x2        y2        z2        x3        y3        z3  NOT-USED  NOT-USED 
      -0.3       0.3    -0.135      -0.3      -0.3      0.39 
$#6 SWTIME      NONE        HG      NAIR      NGAS     NORIF     LCVEL       LCT 
   0.04000     0.005     1.e-4         2         1         1         0         2 
$#7 AIR         NONE      NONE     MWAIR     INITM      AIRA      AIRB      AIRC 
                                   0.028      0.80    27.296   0.00523 
                                   0.032      0.20    25.723   0.01298 
$#8 GASLCM      NONE      NONE     MWGAS      NONE      GASA      GASB      GASC 
         1                        0.0249              29.680   0.00880 
$#9 NODEID    VECTID  ORIFAREA 
      9272         1   1.00e-4 
$ Lagrangian shell structure to be coupled to the inflator gas 
*SET_PART_LIST 
         1       0.0       0.0       0.0       0.0 
         1         2         3 
*DEFINE_VECTOR 
$0.100000E+01,  10.000000000 
$      vid        xt        yt        zt        xh        yh        zh 
         1       0.0       0.0       0.0       0.0       0.0  0.100000 
$ bag penetration ~ 1 mm  <====>  P_coup ~ 500000 pascal ==> ~ 5 atm 
*DEFINE_CURVE 
$     lcid      sidr       sfa       sfo      offa      offo    dattyp 
       321         0       0.0       0.0       0.0       0.0 
$                 a1                  o1 
                 0.0                 0.0 
          0.00100000       5.0000000e+05 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
In this example, LS-DYNA automatically creates the background ALE mesh with: 
NX  =  11 ⇒ 11 elements in the x direction 
NY  =  11 ⇒ 11 Elements in the y direction
NZ  =  9  ⇒ 9 Elements in the z direction
*AIRBAG 
Purpose:  To define two connected airbags which vent into each other. 
  Card 1 
1 
2 
3 
Variable 
AB1 
AB2 
AREA 
Type 
I 
I 
F 
4 
SF 
F 
Default 
none 
none 
none 
none 
5 
6 
7 
8 
PID 
LCID 
IFLOW 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
AB1 
AB2 
First airbag ID, as defined on *AIRBAG card. 
Second airbag ID, as defined on *AIRBAG card. 
AREA 
Orifice area between connected bags. 
LT.0.0:  |AREA| is the load curve ID defining the orifice area
as a function of absolute pressure. 
EQ.0.0:  AREA  is  taken  as  the  surface  area  of  the  part  ID 
defined below. 
SF 
Shape factor. 
LT.0.0:  |SF|  is  the  load  curve  ID  defining  vent  orifice
coefficient as a function of relative time. 
PID 
LCID 
Optional  part  ID  of  the  partition  between  the  interacting  control
volumes.  AREA is based on this part ID.  If PID is negative, the
blockage of the orifice part due to contact is considered, 
Load curve ID defining mass flow rate versus pressure difference, 
see *DEFINE_CURVE.  If LCID is defined AREA, SF and PID are
ignored.   
IFLOW 
Flow direction 
LT.0:  One way flow from AB1 to AB2 only.  
EQ.0:  Two way flow between AB1 and AB2. 
GT.0:  One way flow from AB2 to AB1 only.
*AIRBAG_INTERACTION 
Mass  flow  rate  and  temperature  load  curves  for  the  secondary  chambers  must  be 
defined as null curves, for example, in the DEFINE_CURVE definitions give two points 
(0.0, 0.0) and (10000., 0.0).   
All input options are valid for the following airbag types: 
*AIRBAG_SIMPLE_AIRBAG_MODEL 
*AIRBAG_WANG_NEFSKE 
*AIRBAG_WANG_NEFSKE_JETTING 
*AIRBAG_WANG_NEFSKE_MULTIPLE_JETTING 
*AIRBAG_HYBRID 
*AIRBAG_HYBRID_JETTING 
The  LCID  defining  mass  flow  rate  vs.    pressure  difference  may  additionally  be  used 
with: 
*AIRBAG_LOAD_CURVE 
*AIRBAG_LINEAR_FLUID 
If  the  AREA,  SF,  and  PID  defined  method  is  used  to  define  the  interaction  then  the 
airbags  must  contain  the  same  gas,  i.e.    Cp,  Cv  and  g  must  be  the  same.    The  flow 
between bags is governed by formulae which are similar to those of Wang-Nefske.
*AIRBAG_PARTICLE_{OPTION1}_{OPTION2}_{OPTION3}_{OPTION4} 
Available options include: 
OPTION1 applies to the MPP implementation only. 
MPP 
OPTION2 also applies to the MPP implementation only.  When the DECOMPOSITON 
option is present, LS-DYNA will automatically insert *CONTROL_MPP_DECOMPOSI-
TION_BAGREF 
CONTROL_MPP_DECOMPOSITION_ARRANGE_PARTS 
keywords if they are not already present in the input. 
and 
DECOMPOSITION 
OPTION3  provides  a  means  to  specify  an  airbag  ID  number  and  a  heading  for  the 
airbag. 
ID 
TITLE 
OPTION4: 
MOLEFRACTION  
Purpose:  To define an airbag using the particle method. 
NOTE:  This  model  requires  that  surface  normal  vectors  be  oriented 
inward,  unlike  that  the  traditional  CV  method  for  which  they 
must  point  outward.    To  check  bag  and  chamber  integrity  in  the 
CPM  model  see  the  CPMERR  option  on  the  *CONTROL_CPM 
card. 
MPP Card.  Additional card for MPP keyword option. 
4 
5 
6 
7 
8 
  MPP 
Variable 
1 
SX 
Type 
F 
2 
SY 
F 
3 
SZ 
F 
Default 
none 
none 
none
SX, SY, SZ 
*AIRBAG_PARTICLE 
DESCRIPTION
Scale  factor  for  each  direction  used  during  the  MPP  decomposi-
tion.    For  instance,  increasing  SX  from  1  to  10  will  give  increase
the probability that the model is divided along the 𝑥-direction. 
Title Card.  Additional card for ID or TITLE keyword options. 
TITLE 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BAGID 
Type 
I 
HEADING 
A60 
The BAGID is referenced in, e.g., *INITIAL_AIRBAG_PARTICLE_POSITION. 
  VARIABLE   
DESCRIPTION
BAGID 
Airbag ID.  This must be a unique number. 
HEADING 
Airbag  descriptor.    It  is  suggested  that  unique  descriptions  be
used. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID1 
STYPE1 
SID2 
STYPE2 
BLOCK 
NPDATA 
FRIC 
IRPD 
Type 
I 
Default 
none 
  Card 2 
Variable 
1 
NP 
I 
0 
2 
I 
0 
3 
I 
0 
4 
I 
0 
5 
I 
F 
0.0 
0.0 
6 
7 
I 
0 
8 
UNIT 
VISFLG 
TATM 
PATM 
NVENT 
TEND 
TSW 
Type 
I 
I 
Default  200,000 
0 
I 
0 
F 
F 
293K 
1 atm 
I 
0 
F 
F 
1010 
1010
Optional  control  card.    When  the  card  after  Card  2  begins  with  a  “+”  character  the 
input reader processes it as this card, otherwise this card is skipped. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TSTOP 
TSMTH 
OCCUP 
REBL 
SIDSV 
PSID1 
Type 
F 
F 
F 
Default 
1010 
1msec 
0.1 
I 
0 
I 
I 
none 
none 
Optional unit card.  Additional Cards when Unit = 3. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Mass 
F 
Time 
F 
Length 
F 
Default 
none 
none 
none 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IAIR 
NGAS 
NORIF 
NID1 
NID2 
NID3 
CHM 
CD_EXT 
Type 
Default 
I 
0 
I 
I 
none 
none 
I 
0 
I 
0 
I 
0 
I 
F 
none 
0.
Internal Part Set Cards.  Additional Cards for STYPE2 = 2.  Define SID2 cards, one for 
each internal part or part set. 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SIDUP 
STYUP 
PFRAC 
LINKING 
Type 
I 
I 
F 
I 
Default 
none 
none 
0. 
none 
Heat  Convection  Part  Set  Cards.    Additional  Cards  for  NPDATA > 0.    Define 
NPDATA cards, one for each heat convection part or part set. 
  Card 7 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SIDH 
STYPEH 
HCONV 
PFRIC 
SDFBLK 
KP 
INIP 
Type 
I 
I 
F 
F 
F 
Default 
none 
none 
none 
none 
1.0 
F 
0. 
I 
0 
Vent  Hole  Card.    Additional  Cards  for  NVENT > 0.    Define  NVENT  cards,  one  for 
vent hole. 
  Card 8 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID3 
STYPE3 
C23 
LCTC23 
LCPC23 
ENH_V 
PPOP 
Type 
Default 
I 
0 
I 
F 
none 
1.0 
I 
0 
I 
0 
I 
0 
F 
0.0
Air Card.  Additional Card for IAIR > 0. 
  Card 9 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PAIR 
TAIR 
XMAIR 
AAIR 
BAIR 
CAIR 
NPAIR 
NPRLX 
Type 
F 
F 
F 
F 
F 
F 
Default 
PATM 
TATM 
none 
none 
0.0 
0.0 
I 
0 
I/F 
0 
MOLEFRACTION Card. Additional card for the MOLEFRACTION option. 
  Card 10 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCMASS 
Type 
I 
Default 
none 
Gas Cards.  NGAS additional Cards, one for each gas (card format for ith gas). 
  Card 11 
1 
2 
3 
Variable 
LCMi 
LCTi 
XMi 
Type 
I 
I 
F 
4 
Ai 
F 
5 
Bi 
F 
6 
Ci 
F 
Default 
none 
none 
none 
None 
0.0 
0.0 
7 
8 
INFGi 
I
Orifice Cards.  NORIF additional Cards, one for each orifice (card format for ith orifice).
  Card 12 
1 
Variable 
NIDi 
2 
ANi 
3 
VDi 
4 
5 
6 
7 
8 
CAi 
INFOi 
IMOM 
IANG 
CHM_ID 
Type 
I 
F 
I 
F 
Default 
none 
none 
none 
30 Deg
I 
1 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
SID1 
Part or part set ID defining the complete airbag. 
STYPE1 
Set type: 
EQ.0: Part 
EQ.1: Part set 
SID2 
Part or part set ID defining the internal parts of the airbag. 
STYPE2 
Set type: 
EQ.0: Part 
EQ.1: Part set 
EQ.2: Number of parts to read (Not recommended for general
use)
VARIABLE   
DESCRIPTION
BLOCK 
Blocking.  Block must be set to a two-digit number 
BLOCK = M × 10 + N, 
The  10’s  digit  controls  the  treatment  of  particles  that  escape  due
to deleted elements (particles are always tracked and marked). 
M.EQ.0: Active particle method for which causes particles to be
put back into the bag. 
M.EQ.1: Particles are leaked through vents.  See Remark 3.   
The 1’s digit controls the treatment of leakage. 
N.EQ.0:  Always consider porosity leakage without considering 
blockage due to contact. 
N.EQ.1:  Check  if  airbag  node  is  in  contact  or  not.    If  yes,  1/4
(quad) or 1/3 (tri) of the segment surface will not have
porosity leakage due to contact. 
N.EQ.2:  Same as 1 but no blockage for external vents 
N.EQ.3:  Same as 1 but no blockage for internal vents 
N.EQ.4:  Same as 1 but no blockage for all vents. 
NPDATA 
Number of parts or part sets data. 
FRIC 
IRPD 
Friction factor.  See Remark 2. 
Dynamic scaling of particle radius. 
EQ.0: Off 
EQ.1: On 
NP 
Number of particles.  (Default = 200,000) 
UNIT 
Unit system: 
EQ.0: kg-mm-ms-K 
EQ.1: SI 
EQ.2: tonne-mm-s-K 
EQ.3: User defined units
VISFLG 
*AIRBAG_PARTICLE 
DESCRIPTION
Visible  particles.    This  field  affects  only  the  CPM  database.    See 
Remark 5. 
EQ.0: Default to 1 
EQ.1: Output  particle's  coordinates,  velocities,  mass,  radius,
spin energy, translational energy 
EQ.2: Output reduce data set with coordinates only 
EQ.3: Suppress CPM database 
TATM 
PATM 
Atmospheric temperature.  (Default = 293K) 
Atmospheric pressure.  (Default = 1 ATM) 
NVENT 
Number of vent hole parts or part sets 
TEND 
TSW 
Time when all (NP) particles have entered bag.  (Default = 1010) 
Time  at  which  algorithm  switches 
(Default = 1010) 
to  control  volumes. 
TSTOP 
Time at which front tracking switches from IAIR = 4 to IAIR = 2. 
TSMTH 
OCCUP 
REBL 
SIDSV 
To  avoid  sudden  jumps  in  the  pressure  signal  during  switching
there  is  a  transition  period  during  which  the  front  tracking  is
tapered.  The default time of 1 millisecond will be applied if this
value is set to zero. 
Particles  occupy  OCCUP  percent  of  the  airbag’s  volume.    The 
default value of OCCUP is 10%.  This field can be used to balance
computational cost and signal quality.  OCCUP ranges from 0.001
to 0.1. 
If  the  option  is  ON,  all  energy  stored  from  damping  will  be
evenly  distributed  as  vibrational  energy  to  all  particles.    This 
improves the pressure calculation in certain applications. 
EQ.0:  Off (Default) 
EQ.1:  On 
Part  set  ID  for  internal  shell  part.    The  volume  occupied  by  this
part is excluded from the bag volume.  These internal parts must
be consistently orientated for the excluded volume to be correctly
calculated.
VARIABLE   
PSID1 
DESCRIPTION
Part  set  ID  for  external  parts  which  have  normal  pointed 
outward.  This option is usually used with airbag integrity check
while  there  are  two  CPM  bags  connected  with  bag  interaction.
Therefore,  one  of  the  bag  can  have  the  correct  shell  orientation
but  the  share  parts  for  the  second  bag  will  have  wrong 
orientation.  This option will automatically flip the parts defined
in this set in the second bag during integrity checking. 
Mass, Time, 
Length 
Conversion factor from current unit to MKS unit.  For example, if
the  current  unit  is  using  kg-mm-ms,  the  input  should  be 
1.0, 0.001, 0.001 
IAIR 
Initial gas inside bag considered: 
EQ.0:  No 
EQ.1:  Yes, using control volume method. 
EQ.-1:  Yes, using control volume method.  In this cake ambient
air enters the bag when PATM is greater than bag pres-
sure. 
EQ.2:  Yes, using the particle method. 
EQ.4:  Yes,  using  the  particle  method.    Initial  air  particles  are
used  for  the  gas  front  tracking  algorithm  but  they  do
not apply forces when they collide with a segment.  In-
stead, a uniform pressure is applied to the airbag based 
on  the  ratio  of  air  and  inflator  particles.    In  this  case
NPRLX must be negative so that forces are not applied
by the initial air. 
NGAS 
Number of gas components 
NORIF 
Number of orifices 
NID1 - NID3 
Three  nodes  defining  a  moving  coordinate  system  for  the 
direction  of  flow  through  the  gas  inlet  nozzles  (Default = fixed 
system) 
CHM 
Chamber ID used in *DEFINE_CPM_CHAMBER.  See Remark 7. 
CD_EXT 
Drag  coefficient  for  external  air.    If  the  value  is  not  zero,  the
inertial effect from external air will be considered and forces will
be applied in the normal direction on the exterior airbag surface.
SIDUP 
*AIRBAG_PARTICLE 
DESCRIPTION
Part or part set ID defining the internal parts that pressure will be
applied  to.    This  internal  structure  acts  as  a  valve  to  control  the 
external vent hole area.  Pressure will be applied only after switch
to UP (uniform pressure) using TSW. 
STYUP 
Set type: 
EQ.0: Part 
EQ.1: Part set 
PFRAC 
LINKING 
Fraction  of  pressure  to  be  applied  to  the  set  (0.0  to  1.0).    If
PFRAC = 0, no pressure is applied to internal parts. 
Part  ID  of  an  internal  part  that  is  coupled  to  the  external  vent
definition.  The minimum area of this part or the vent hole will be 
used for actual venting area. 
SIDH 
Part or part set ID defining part data. 
STYPEH 
Set type: 
EQ.0: Part 
EQ.1: Part set 
HCONV 
Heat  convection  coefficient  used  to  calculate  heat  loss  from  the
airbag external surface to ambient (W/K/m2).  See *AIRBAG_HY-
BRID developments (Resp.  P.O.  Marklund). 
LT.0: |HCONV|  is  a  load  curve  ID  defines  heat  convection
coefficient as a function of time. 
PFRIC 
Friction factor.  PFRIC Defaults to FRIC from 1st card 7th field. 
SDFBLK 
Scale  down  factor  for  blockage  factor  (Default = 1,  no  scale 
down).  The valid factor will be (0,1].  If 0, it will set to 1. 
KP 
INIP 
Thermal conductivity of the part.  See Remark 9. 
Place initial air particles on surface. 
EQ.0: yes (default) 
EQ.1: no 
This feature exclude surfaces from initial particle placement.  This
option  is  useful  for  preventing  particles  from  being  trapped
between adjacent fabric layers.
VARIABLE   
DESCRIPTION
SID3 
Part or part set ID defining vent holes. 
STYPE3 
Set type: 
EQ.0: Part 
EQ.1: Part set which each part being treated separately 
EQ.2: Part set and all parts are treated as one vent.  See Remark 
13. 
    GE..0:  Vent  hole  coefficient,  a  parameter  of  Wang-Nefske 
leakage.  A value between 0.0-1.0 can be input, default = 1.0.  See 
Remark 1. 
    LT.0: ID for *DEFINE_CPM_VENT 
Load  curve  defining  vent  hole  coefficient  as  a  function  of  time.
LCTC23  can  be  defined  through  *DEFINE_CURVE_FUNCTION. 
If omitted a curve equal to 1 used.  See Remark 1. 
C23 
LCTC23 
LCPC23 
Load  curve  defining  vent  hole  coefficient  as  a  function  of
pressure.  If omitted a curve equal to 1 is used.  See Remark 1. 
ENH_V 
Enhanced venting option.  See Remark 8. 
EQ.0: Off (default) 
EQ.1: On 
EQ.2: Two  way  flow  for  internal  vent;  treated  as  hole  for
external vent  
Pressure  difference  between  interior  and  ambient  pressure 
(PATM)  to  open  the  vent  holes.    Once  the  vents  are  open,  they
will stay open. 
Initial pressure inside bag.  (Default PAIR = PATM) 
Initial temperature inside bag.  (Default, TAIR = TATM) 
PPOP 
PAIR 
TAIR 
XMAIR 
Molar mass of gas initially inside bag. 
AAIR - CAIR 
Constant, linear, and quadratic heat capacity parameters. 
NPAIR 
Number of particle for air.  See Remark 6.
*AIRBAG_PARTICLE 
DESCRIPTION
NPRLX 
Number of cycles to reach thermal equilibrium.  See Remark 6. 
LT.0: If  more  than  50%  of  the  collision  to  fabric  is  from  initial
air  particle,  the  contact  force  will  not  apply  to  the  fabric
segment in order to keep its original shape. 
If the number contains “.”, “e” or “E”, NPRLX will treated as an
end time rather than as a cycle count. 
LCMASS 
Total mass flow rate curve for the MOLEFRACTION option. 
LCMi 
LCTi 
XMi 
Ai - Ci 
INFGi 
NIDi 
ANi 
VDi 
flow  rate  curve 
Mass 
the 
MOLEFRACTION  option  is  used,  then  it  is  the  time  dependent
molar fraction of the total flow for gas component i. 
for  gas  component 
i,  unless 
Temperature curve for gas component i. 
Molar mass of gas component i. 
Constant,  linear,  and  quadratic  heat  capacity  parameters  for  gas 
component i. 
Inflator ID for this gas component (Defaults to 1). 
Node  ID/Shell  ID  defining  the  location  of  nozzle i.    See  Remark 
12. 
Area of nozzle i.  (Default: all nozzles are assigned the same area)
GT.0:  Vector ID.  Initial direction of gas inflow at nozzle 𝑖. 
LT.0:  Values  in  the  NIDi  fields  are  interpreted  as  shell  IDs. 
See Remark 12. 
EQ.-1:  direction of gas inflow is using shell normal 
EQ.-2:  direction of gas inflow is in reversed shell normal 
CAi 
Cone  angle  in  degrees  (Defaults  to  30  degrees).    This  option  is 
used only when IANG equal to 1. 
INFOi 
Inflator ID for this orifice.  (Default = 1) 
IMOM 
Inflator reaction force (R5.1.1 release and later). 
EQ.0: Off 
EQ.1: On
VARIABLE   
IANG 
DESCRIPTION
Activation  for  cone  angle  to  use  for  friction  calibration(not
normally  used;  eliminates  thermal  energy  of  particles  from
inflator). 
EQ.0: Off (Default) 
EQ.1: On 
CHM_ID 
Chamber  ID  where  the  inflator  node  resides.    Chambers  are
defined using the *DEFINE_CPM_CHAMBER keyword. 
Remarks: 
1.  Formula for Total Vent Hole Coefficient.  The value must be between 0 and 1. 
Total vent hole coefficient = min(max(C23 × LCTC23 × LCPC23, 0), 1) 
2.  Surface Roughtness.  Friction factor to simulate the surface roughness.  If the 
surface  is  frictionless  the  particle  incoming  angle  𝛼1is  equal  to  the  deflection 
angle 𝛼2. 
Considering surface roughness  𝐹r and the total angle 𝛼 will have the following 
relationships: 
For the special case when, 
0 ≤ 𝐹r ≤ 1 
 𝛼 = 𝛼1 + 𝛼2 
𝐹r = 1 
the incoming particle will bounce back from its incoming direction, 
 𝛼 = 0. 
For,  −1 ≤ 𝐹𝑟 < 0,  particles  will  bounce  towards  the  surface  by  the  following 
relationship 
𝛼 = 2 [𝛼1 − 𝐹𝑟 (
−
𝛼1
)]. 
3.  Blocking  and  BLOCK  Field.    Setting  the  10’s  digit  to  1  allows  for  physical 
holes in an airbag.  In this case, particles that are far away from the airbag are
disabled.  In most case, these are particles that have escaped through unclosed 
surfaces due to physical holes, failed elements, etc.  This reduces the bucket sort 
search distance. 
4.  Convection Energy Balance.  The change in energy due to convection is given 
by  
Where, 
d𝐸
d𝑡
= 𝐴 × HCONV × (𝑇bag − 𝑇atm). 
𝐴  = is part area. 
HCONV = user defined heat convection coefficient. 
𝑇bag = the weighted average temperature impacting particles. 
𝑇atm = aambient temperature. 
5.  Output  Files.    Particle  time  history  data  is  always  output  to  d3plot  database 
now.    LS-PrePost  2.3  and  later  can  display  and  fringe  this  data.    In  order  to 
reduce  runtime  memory  requirements,  VISFLG  should  be  set  to  0  (disabled).  
For  LS-DYNA  971  R6.1  and  later,  VISFLG  only  affects  Version  4  CPM  output 
. 
6.  Spatial  Distribution  Equilibration  for  Airbag  Particles.    Total  number  of 
particles  used  in  each  card  is  NP  +  NPAIR.    Since  the  initial  air  particles  are 
placed  at  the  surface  of  the  airbag  segments  with  correct  velocity  distribution 
initially,  particles  are  not  randomly  distributed  in  space.    It  requires  a  finite 
number  of  relaxation  cycles,  NPRLX,  to  allow  particles  to  move  and  produce 
better spatial distribution. 
Since  the  momentum  and  energy  transfer  between  particles  are  based  on  per-
fect  elastic  collision,  CPM  solver  would  like  to  keep  similar  mole  per  particle 
between inflator and initial air particles.  CPM solver will check the following 
factor. 
factor = ∣1 −
mole per particle of initial air
∣ 
mole per particle of inflator gas
If the factor is more than 10% apart, code will issue the warning message with 
the tag, (SOL+1232) and provide the suggested NPAIR value.  User needs make 
decision to adjust the NPAIR value based on the application.  For example, user 
setup only initial air without any inflator gas for certain impact analysis should 
ignore this warning message. 
7.  Remark  Concerning  *DEFINE_CPM_CHAMBER.    By  default  initial  air 
particles will be evenly placed on airbag segments which cannot sense the local 
volume.  This will create incorrect pressure field if the bag has several distinct 
pockets.    *DEFINE_CPM_CHAMBER  allows  the  user  to  initialize  air  particles
by volume ratios of regions of airbag.  The particles will be distributed propor-
tional to the defined chamber volume to achieve better pressure distribution. 
8.  Enhanced Venting.   When enhanced venting is on, the vent hole’s equivalent 
radius  𝑅eq  will  be  calculated.    Particles  within  𝑅eq  on  the  high  pressure  side 
from  the  vent  hole  geometry  center  will  be  moved  toward  the  hole.    This  will 
increase the collision frequency near the vent for particles to detect small struc-
tural features and produce better flow through the vent hole. 
ENH_V  equals  1,  particles  are  flow  from  high  to  low  pressure  only.    EHN_V 
equals 2, particles can flow in both directions for internal vent. 
Particles encountering external vents are released.  The ambient pressure is not 
taken into account and the particle will be released regardless the value of the 
pressure  in  the  bag/chamber.    Therefore,  the  vent  rate  will  be  sensitive  to  the 
vent location. 
9.  Effective Convection Heat Transfer Coefficient.  If the thermal conductivity, 
KP, is given, then the effective convection heat transfer coefficient is given by 
𝐻eff = (
1.0
HCONV
+
shell thickness
KP
)
−1
, 
where the part thickness comes from the SECTION database.  If KP is not given, 
𝐻eff defaults to HCONV. 
10.  MOLEFRACTION  Option.    Without  the  MOLEFRACTION  option,  a  flow  rate 
is specified for each species on the LCMi fields of   Card 11.  With the MOLE-
FRACTION option the total mass flow rate is specified in the LCMASS field on 
Card 10 and the molar fractions are specified in the LCMi fields of   Card 
11. 
11.  User Defined Units.   If  UNIT = 3  is  used, there  is  no  default  value  for  TATM 
and  PATM  and  user  should  provide  the  proper  values.    User  also  needs  to 
provide  unit  conversion  factors  for  code  to  set  correct  universal  gas  constant 
and some other variables used in the code. 
12.  Shell Based Nozzle.  Node ID and shell ID based nozzle should not be used in 
the same airbag definition.  The nozzle location is taken to be at the center of the 
shell and the initial nozzle direction can be defined by shell’s normal or by its 
reversed normal.  This vector is transforms with the moving coordinate system 
defined by NID1 - NID3.  The nozzle area is set on the ANi fields and shell area 
is not taken into account; therefore, the mass flowrate distribution with shells is 
determined in the same way as it is with nozzles defined by nodes.  
13.  Merge Part Set for Vent.  The first part in the set is designated as the master.  
All  remaining  parts  are  merged  into  the  master  so  that  enhanced  venting  is
treated  correctly.    ABSTAT_CPM  output  will  be  associated  with  the  master 
part.    This  option  has  the  same  effect  as  manually  merging  elements  into  the 
master part.
*AIRBAG_REFERENCE_GEOMETRY_{OPTION}_{OPTION}_{OPTION} 
Available options include: 
<BLANK> 
BIRTH 
RDT 
ID 
Purpose:    If  the  reference  configuration  of  the  airbag  is  taken  as  the  folded  configura-
tion,  the  geometrical  accuracy  of  the  deployed  bag  will  be  affected  by  both  the 
stretching  and  the  compression  of  elements  during  the  folding  process.    Such  element 
distortions  are  very  difficult  to  avoid  in  a  folded  bag.    By  reading  in  a  reference 
configuration  such  as  the  final  unstretched  configuration  of  a  deployed  bag,  any 
distortions  in  the  initial  geometry  of  the  folded  bag  will  have  no  effect  on  the  final 
geometry  of  the  inflated  bag.    This  is  because  the  stresses  depend  only  on  the 
deformation gradient matrix: 
𝐹𝑖𝑗 =
∂𝑥𝑖
∂𝑋𝑗
where the choice of 𝑋𝑗 may coincide with the folded or unfold configurations.  It is this 
unfolded configuration which may be specified here. 
Note  that  a  reference  geometry  which  is  smaller  than  the  initial  airbag  geometry  will 
not induce initial tensile stresses. 
If a liner is included and the parameter LNRC set to 1 in *MAT_FABRIC, compression is 
disabled  in  the  liner  until  the  reference  geometry  is  reached,  i.e.,  the  fabric  element 
becomes tensile. 
When the BIRTH option is specified an additional card setting the BIRTH parameter is 
activated.    The  BIRTH  parameter  specifies  a  critical  time  value  before  which  the 
reference  geometry  is  not  used.    Until  the  BIRTH  time  is  reach  the  input  geometry  is 
used  for  (1)  inflating  the  airbag  and  for  (2)  determining  the  time step  size,  even  when 
the RDT option is set.
NOTE:  This card does not support multiple birth times.  The 
last BIRTH value read will be used for all preceding 
*AIRBAG_REFERENCE_GEOMETRY_BIRTH defini-
tions.  RGBRTH in *MAT_FABRIC supports a mate-
rial dependent birth time. 
When  the  RDT  option  is  active  the  time  step  size  will  be  based  on  the  reference 
geometry  once  the  solution  time  exceeds  the  birth  time.    This  option  is  useful  for 
shrunken  bags  where  the  bag  does  not  carry  compressive  loads  and  the  elements  can 
freely expand before stresses develop.  If this option is not specified, the time step size 
will be based on the current configuration and will increase as the area of the elements 
increase.  The default may be much more expensive but possibly more stable. 
ID card.  Additional card for keyword option ID. 
ID 
Variable 
1 
ID 
Type 
I 
2 
SX 
F 
3 
SY 
F 
4 
SZ 
F 
5 
6 
7 
8 
NIDO 
I 
Default 
none 
1.0 
1.0 
1.0 
1st NID 
Birth card.  Additional card for keyword option BIRTH. 
Birth 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BIRTH 
Type 
F 
Default 
0.0
Node  Cards.    For  each  node  ID  having  an  associated  reference  position  include  an 
additional card in format 2.  The next “*” keyword card terminates this input.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
NID 
Type 
I 
X 
F 
Default 
none 
0. 
Remark 
Y 
F 
0. 
Z 
F 
0. 
  VARIABLE   
DESCRIPTION
ID 
Card ID 
SX, SY, SZ 
Scale factor in each direction 
NIDO 
Node  ID  for  origin.    Default  is  the  first  node  ID  defined  in  this
keyword. 
BIRTH 
Time at which the reference geometry activates (default = 0.0) 
NID 
X 
Y 
Z 
Node  ID  for  which  a  reference  configuration  is  defined.    Nodes
defined in this section must also appear under the *NODE input.
It  is  only  necessary  to  define  the  reference  coordinates  of  nodal
points, if their coordinates are different than those defined in the 
*NODE section. 
𝑥 coordinate 
𝑦 coordinate 
𝑧 coordinate
*AIRBAG_SHELL_REFERENCE_GEOMETRY_{OPTION}_{OPTION} 
Available options include: 
<BLANK> 
RDT 
ID 
Purpose:    Usually,  the  input  in  this  section  is  not  needed;  however,  sometimes  it  is 
convenient to use disjoint pre-cut airbag parts to define the reference geometries.  If the 
reference  geometry  is  based  only  on  nodal  input,  this  is  not  possible  since  in  the 
assembled airbag the boundary nodes are merged between parts.  By including the shell 
connectivity  with  the  reference  geometry,  the  reference  geometry  can  be  based  on  the 
pre-cut airbag parts instead of the assembled airbag.  The elements, which are defined 
in  this  section,  must  have  identical  element  ID’s  as  those  defined  in  the  *ELEMENT_-
SHELL input, but the nodal ID’s, which may be unique, are only used for the reference 
geometry.    These  nodes  are  defined  in  the  *NODE  section  but  can  be  additionlly 
defined  in  *AIRBAG_REFERENCE_GEOMETRY.    The  element  orientation  and  n1-n4 
ordering must be identical to the *ELEMENT_SHELL input. 
When  the  RDT  option  is  active  the  time  step  size  will  be  based  on  the  reference 
geometry  once  the  solution  time  exceeds  the  birth  time  which  can  be  defined  by 
RGBRTH of *MAT_FABRIC. 
ID card.  Additional card for keyword option ID. 
  Card 1 
Variable 
1 
ID 
Type 
I 
2 
SX 
F 
3 
SY 
F 
4 
SZ 
F 
5 
NID 
I 
Default 
none 
1.0 
1.0 
1.0 
See List
6 
7
Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
EID 
PID 
N1 
N2 
N3 
N4 
Type 
I 
I 
I 
I 
I 
I 
Default 
none  none  none  none  none  none 
  VARIABLE   
DESCRIPTION
ID 
Card ID 
SX, SY, SZ 
Scale factor in each direction 
NID 
EID 
PID 
N1 
N2 
N3 
N4 
Node  ID  for  origin.    Default  is  the  first  node  ID  defined  in  this
keyword. 
Element ID 
Optional  part  ID,  see  *PART,  the  part  ID  is  not  used  in  this
section. 
Nodal point 1 
Nodal point 2 
Nodal point 3 
Nodal point 4
ALE does not support implicit time integration nor does it support dynamic relaxation.  
Furthermore, except for ALE formulation 5, which does support contact, ALE does not, in 
general, support contact. 
In three dimensions, ALE supports only one-point solid elements.  These solid elements 
can  either  be  hexahedral,  pentahedral,  or  tetrahedral.    Pentahedrons  and  tetrahedrons 
are  treated  as  degenerate  hexahedron  elements.    For  each  ALE  multi-material,  strain 
and stress is evaluated in each solid element at a single integration point.  In this sense, 
the ALE element formulation is equivalent to ELEFORM 1 solid formulation. 
Keywords for the ALE structured solver. 
*ALE_STRUCTURED_MESH 
*ALE_STRUCTURED_MESH_CONTROL_POINTS 
Input  required  for  LS-DYNA’s  Arbitrary-Lagrangian-Eulerian  capability  is  defined 
using *ALE cards.  The keyword cards in this section are defined in alphabetical order: 
*ALE_AMBIENT_HYDROSTATIC 
*ALE_COUPLING_NODAL_CONSTRAINT 
*ALE_COUPLING_NODAL_DRAG 
*ALE_COUPLING_NODAL_PENALTY 
*ALE_COUPLING_RIGID_BODY 
*ALE_ESSENTIAL_BOUNDARY 
*ALE_FAIL_SWITCH_MMG 
*ALE_FRAGMENTATION 
*ALE_FSI_PROJECTION 
*ALE_FSI_SWITCH_MMG_{OPTION} 
*ALE_FSI_TO_LOAD_NODE 
*ALE_MULTI-MATERIAL_GROUP 
*ALE_REFERENCE_SYSTEM_CURVE
*ALE_REFERENCE_SYSTEM_NODE 
*ALE_REFERENCE_SYSTEM_SWITCH 
*ALE_REFINE 
*ALE_SMOOTHING 
*ALE_TANK_TEST 
*ALE_UP_SWITCH 
For other input information related to the ALE capability, see keywords: 
*ALE_TANK_TEST 
*BOUNDARY_AMBIENT_EOS 
*CONSTRAINED_EULER_IN_EULER 
*CONSTRAINED_LAGRANGE_IN_SOLID 
*CONTROL_ALE 
*DATABASE_FSI 
*INITIAL_VOID 
*INITIAL_VOLUME_FRACTION 
*INITIAL_VOLUME_FRACTION_GEOMETRY 
*SECTION_SOLID 
*SECTION_POINT_SOURCE_FOR_GAS_ONLY 
*SECTION_POINT_SOURCE_MIXTURE 
*SET_MULTIMATERIAL_GROUP_LIST 
*CONSTRAINED_EULER_IN_EULER 
For a single gaseous material: 
*EOS_LINEAR_POLYNOMIAL 
*EOS_IDEAL_GAS
For multiple gaseous materials: 
*MAT_GAS_MIXTURE 
*INTIAL_GAS_MIXTURE
*ALE_AMBIENT_HYDROSTATIC 
Purpose:    When  an  ALE  model  contains  one  or  more  ambient  (or  reservoir-type)  ALE 
parts  (ELFORM = 11  and  AET = 4),  this  command  may  be  used  to  initialize  the 
hydrostatic  pressure  field  in  the  ambient  ALE  domain  due  to  gravity.    The  *LOAD_-
BODY_{OPTION} keyword must be defined.  The associated *INITIAL_HYDROSTAT-
IC_ALE  keyword  may  be  used  to  define  a  similar  initial  hydrostatic  pressure  field  for 
the regular ALE domain (not reservoir-type region). 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ALESID 
STYPE 
VECID 
GRAV 
PBASE  RAMPTLC 
Type 
I 
Default 
none 
  Card 2 
1 
I 
0 
2 
I 
none 
3 
I 
0 
4 
I 
0 
5 
I 
0 
6 
7 
8 
Variable 
NID 
MMGBL 
Type 
I 
I 
Default 
None 
none 
  VARIABLE   
ALESID 
DESCRIPTION
ALESID  defines  the  reservoir-type  ALE  domain/mesh  whose 
hydrostatic  pressure  field  due  to  gravity  is  being  initialized  by
this keyword.  See Remark 4. 
STYPE 
ALESID set type.  See Remark 4. 
EQ.0: Part set ID (PSID), 
EQ.1: Part ID (PID) ), 
EQ.2: Solid set ID (SSID). 
VECID 
Vector ID of a vector defining the direction of gravity.
VARIABLE   
DESCRIPTION
GRAV 
PBASE 
Magnitude  of  the  Gravitational  acceleration.    For  example,  in
metric units the value is usually set to 9.80665 m/s2. 
Nominal  or  reference  pressure  at  the  top  surface  of  all  fluid
layers.    By  convention,  the  gravity  direction  points  from  the  top
layer to the bottom layer.  Each fluid layer must be represented by
an  ALE  multi-material  group  ID  (AMMGID  or  MMG).    See
Remark 1. 
RAMPTLC 
A  ramping  time  function  load  curve  ID.    This  curve  (via  *DE-
FINE_CURVE) defines how gravity is ramped up as a function of
time.  Given GRAV value above, the curve’s ordinate varies from
0.0 to 1.0, and its abscissa is the (ramping) time.  See Remark 2. 
NID 
Node ID defining the top of an ALE fluid (AMMG) layer. 
MMGBL 
AMMG  ID  of  the  fluid  layer  immediately  below  this  NID.    Each
node  is  defined  in  association  with  one  AMMG  layer  below  it. 
See Remark 4. 
Remarks: 
1.  Pressure in Multi-Layer Fluids.  For models using multi-layer ALE Fluids the 
pressure at the top surface of the top fluid layer is set to PBASE and the hydro-
static pressure is computed as following 
𝑁layers
𝑃 = 𝑃base + ∑ 𝜌𝑖𝑔ℎ𝑖
 . 
𝑖=1
2.  Hydrostatic Pressure Ramp Up.  If RAMPTLC is activated (i.e.  not equal to 
“0”), then the hydrostatic pressure is effectively ramped up over a user-defined 
duration  and  kept  steady.    When  this  load  curve  is  defined,  do  not  define  the 
associated  *INITIAL_HYDROSTATIC_ALE  card  to  initialize  the  hydrostatic 
pressure  for  the  non-reservoir  ALE  domain.    The  hydrostatic  pressure  in  the 
regular ALE region will be initialized indirectly as a consequence of the hydro-
static  pressure  generated  in  the  reservoir-type  ALE  domain.    The  same  load 
curve  should  be  used  to  ramp  up  gravity  in  a  corresponding  *LOAD_-
BODY_(OPTION)  card.    Via  this  approach,  any  submerged  Lagrangian  struc-
ture  coupled  to  the  ALE  fluids  will  have  time  to  equilibrate  to  the  proper 
hydrostatic condition. 
3.  Limitation  on  EOS  Model.    The  keyword  only  supports  *EOS_GRUNEISEN 
and  *EOS_LINEAR_POLYNOMIAL, but only inthe following two cases,
𝑐4 = 𝑐5 > 0,
𝑐3 = 𝑐4 = 𝑐5 = 𝑐6 = 0,
𝑐1 = 𝑐2 = 𝑐3 = 𝑐6 = 0,
𝐸0 = 0
𝑉0 = 0.
4.  Structured  ALE  usage.      When  used  with  structured  ALE,  PART  and  PART 
set options might not make too much sense.  This is because all elements inside 
a structured ALE mesh are assigned to one single PART ID.  In the Structured 
ALE case,  we should  generate a solid set which  contains those ALE boundary 
elements we want to prescribe hydrostatic pressures on.  It is done by using the 
*SET_SOLID_GENERAL  keyword  with  SALECPT  option.    And  then  use  the 
STYPE=2 option (Solid element set ID). 
Example: 
Model Summary: Consider a model consisting of 2 ALE parts, air on top of water. 
H3  =  AMMG1  =  Air part above 
H4  =  AMMG2  =  Water part below
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
$ ALE materials (fluids) listed from top to bottom: 
$ 
$ NID AT TOP OF A LAYER SURFACE         ALE MATERIAL LAYER BELOW THIS NODE 
$ TOP OF 1st LAYER -------> 1681        ---------------------------------------- 
$                                       Air above   = PID 3 = H3 = AMMG1 (AET=4) 
$ TOP OF 2nd LAYER -------> 1671        ---------------------------------------- 
$                                       Water below = PID 4 = H4 = AMMG2 (AET=4) 
$ BOTTOM -------------------->          ---------------------------------------- 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
*ALE_AMBIENT_HYDROSTATIC 
$   ALESID     STYPE     VECID      GRAV     PBASE   RAMPTLC 
        34         0        11   9.80665  101325.0         9 
$      NID    MMGBL 
      1681         1 
      1671         2 
*SET_PART_LIST 
        34 
         3         4 
*ALE_MULTI-MATERIAL_GROUP 
         3         1 
         4         1 
*DEFINE_VECTOR 
$      VID        XT        YT        ZT        XH        YH        ZH       CID 
        11       0.0       1.0       0.0       0.0       0.0       0.0 
*DEFINE_CURVE 
         9 
               0.000               0.000 
               0.001               1.000 
              10.000               1.000 
*LOAD_BODY_Y 
$     LCID        SF    LCIDDR        XC        YC        ZC 
         9   9.80665         0       0.0       0.0       0.0 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8
*ALE_COUPLING_NODAL_CONSTRAINT_{OPTION} 
Available options include: 
<BLANK> 
ID 
TITLE 
Purpose:    This  keyword  activates  constraint  coupling  between  ALE  materials  (master) 
and  non-ALE  nodes.    The  slave  nodes  may  belong  to  Lagrangian  solid,  shell,  beam, 
thick  shell,  or  discrete  sphere    elements.    In 
contrast  to  *ALE_COUPLING_NODAL_PENALTY,  caution  should  be  exercised  in 
connection  with  EFG  and  SPH  nodes,  as  meshless  methods  generally  do  not  satisfy 
essential boundary conditions, leading to energy dissipation.  
This  keyword  requires  a  3D  ALE  formulation.    It  is,  there-
fore,  incompatible  with  parts  defined  using  *SECTION_-
ALE2D or *SECTION_ALE1D. 
If  a  title  is  not  defined  LS-DYNA  will  automatically  create  an  internal  title  for  this 
coupling definition.  
Title Card.  Additional card for TITLE and ID keyword options. 
Title 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
COUPID 
Type 
I 
TITLE 
A70 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SLAVE  MASTER 
SSTYP 
MSTYP 
CTYPE 
MCOUP 
Type 
I 
I 
Default 
none 
none 
I 
0 
I 
0 
I 
1 
I
Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
START 
END 
Type 
Default 
F 
0 
F 
1.0E10 
FRCMIN 
F 
0.5 
  VARIABLE   
COUPID 
DESCRIPTION
Coupling  (card)  ID  number  (I10).    If  not  defined,  LSDYNA  will
assign  an  internal  coupling  ID  based  on the  order of  appearance
in the input deck. 
TITLE 
A description of this coupling definition (A70). 
SLAVE 
Slave  set  ID  defining  a  part,  part  set  or  segment  set  ID  of  the 
Lagrangian or slave structure .  See Remark 1.   
MASTER 
Master set ID defining a part or part set ID of the ALE or master 
solid elements . 
SSTYP 
Slave set type of “SLAVE”: 
EQ.0: part set ID (PSID). 
EQ.1: part ID (PID). 
EQ.2: segment set ID (SGSID). 
EQ.3: node set ID (NSID). 
MSTYP 
Master set type of “MASTER”: 
EQ.0: part set ID (PSID). 
EQ.1: part ID (PID). 
CTYPE 
Coupling type: 
EQ.1: constrained velocity only. 
EQ.2: constrained acceleration and velocity. 
MCOUP 
Multi-material option . 
EQ.0: couple with all multi-material groups,
VARIABLE   
DESCRIPTION
LT.0:  MCOUP must be an integer.  –MCOUP refers to a set ID 
of an ALE multi-material groups defined in *SET_MUL-
TI-MATERIAL_GROUP. 
START 
Start time for coupling. 
END 
End time for coupling. 
FRCMIN 
Only  to  be  used  with  nonzero  MCOUP.    Minimum  volume
fraction  of  the  fluid  materials  included  in  the  list  of  AMMGs  to
activate coupling.  Default value is 0.5.  
Remarks: 
When  MCOUP  is  a  negative  integer,  say  for  example  MCOUP = -123,  then  an  ALE 
multi-material  set-ID  (AMMSID)  of  123  must  exist.    This  is  an  ID  defined  by  a  *SET_-
MULTI-MATERIAL_GROUP_LIST card.
*ALE_COUPLING_NODAL_DRAG 
Available options include: 
<BLANK> 
ID 
TITLE 
Purpose:  This command provides a coupling mechanism to model the drag interaction 
between  ALE  fluids,  which  provide  the  master  elements,  and  discrete  element  forms, 
which comprise the slave nodes.  The slave nodes are assumed to be of spherical shape 
being  either  SPH  elements,  or  discrete  elements  (*ELEMENT_DISCRETE_SPHERE).  
The  coupling  forces  are  proportional  to  the  relative  speed  between  the  fluid  and 
particles plus the buoyancy force due to gravitational loading. 
This  keyword  requires  a  3D  ALE  formulation.    It  is,  there-
fore,  incompatible  with  parts  defined  using  *SECTION_-
ALE2D or *SECTION_ALE1D. 
If  a  title  is  not  defined,  LS-DYNA  will  automatically  generate  an  internal  title  for  this 
coupling definition.  
Title Card.  Additional card for TITLE and ID keyword options. 
Title 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
COUPID 
Type 
I 
TITLE 
A70 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SLAVE  MASTER 
SSTYP 
MSTYP 
Type 
I 
I 
Default 
none 
none 
I 
0 
I
Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
START 
END 
FCOEF 
DIRECG 
GRAV 
Type 
Default 
F 
0 
F 
1.0E10 
F 
1.0 
I 
F 
none 
0.0 
  VARIABLE   
COUPID 
DESCRIPTION
Coupling  (card)  ID  number  (I10).    If  not  defined,  LSDYNA  will
assign  an  internal  coupling  ID  based  on the  order of  appearance
in the input deck. 
TITLE 
A description of this coupling definition (A70). 
SLAVE 
Slave  set  ID  defining  a  part,  part  set  or  segment  set  ID  of  the 
Lagrangian or slave structure . 
MASTER 
Master set ID defining a part or part set ID of the ALE or master 
solid elements . 
SSTYP 
Slave set type of “SLAVE”: 
EQ.0: part set ID (PSID). 
EQ.1: part ID (PID). 
EQ.2: segment set ID (SGSID). 
EQ.3: node set ID (NSID). 
MSTYP 
Master set type of “MASTER”: 
EQ.0: part set ID (PSID). 
EQ.1: part ID (PID). 
START 
Start time for coupling. 
END 
End time for coupling.
FCOEF 
*ALE_COUPLING_NODAL_DRAG 
DESCRIPTION
Drag  coefficient  scale  factor  or  function  ID  to  calculate  drag
coefficient 
GT.0: Drag coefficient scale factor. 
LT.0:  The  absolute  value  of  FCOEF  is  the  Function  ID  of  the
user  provided  function  to  calculate  drag  coefficient;  See
Remark 1. 
DIRECG 
Gravity force direction.  
EQ.1:  Global x direction 
EQ.2:  Global y direction 
EQ.3: Global z direction 
GRAV 
Gravity value.  This value is used to calculate buoyance force. 
Remarks: 
1.  Drag  Coupling  Force.    The  drag  coupling  force  in  between  the  particles  and 
ALE fluids takes the following form. 
𝐹drag = 𝑐drag × 1
𝜌𝑣2 × 1
𝜋𝑑2 
where  𝑐drag  is  the  drag  coefficient,  𝜌  the  fluid  density  in  which  the  particle  is 
submerged,  𝑣  the  relative  velocity  between  the  particle  and  the  fluid,  𝑑  the 
diameter of the particle. 
The default drag coefficient is a function of Reynolds’s number and calculated 
by using the following formula: 
𝑐drag =
⎜⎛0.63 +
⎝
. 
4.8
⎟⎞
√Re⎠
Users can define their own function of drag coefficient.  To do that, one needs to 
define a function using *DEFINE_FUNCTION and assign the negative function 
ID to FCOEF flag.
An  example  is  provided  below  to  illustrate  the  setup.    It  is  equivalent  to  the 
default drag coefficient calculation.  
*ALE_COUPLING_NODAL_DRAG 
     10001         1         3         1 
                                     -10                             3      9.81 
*DEFINE_FUNCTION 
        10 
float cd(float re) 
{ 
  float cd; 
  cd=(0.63+4.8/sqrt(re))*(0.63+4.8/sqrt(re)); 
  if (cd > 2.0) cd = 2.0; 
  return cd; 
}
*ALE_COUPLING_NODAL_PENALTY 
Available options include: 
<BLANK> 
ID 
TITLE 
Purpose:    This  command  provides  a  penalty  coupling  mechanism  between  ALE 
materials  (master)  and  non-ALE  nodes  (slave).    The  slave  nodes  may  belong  to 
Lagrangian solid, shell, beam, thick shell, or discrete (*ELEMENT_DISCRETE_SPHERE) 
elements.    In  contrast  to  *ALE_COUPLING_NODAL_CONSTRAINT,  SPH  and  EFG 
nodes are supported. 
This  keyword  is  incompatible  with  parts  that  use  *SEC-
TION_ALE2D  or  *SECTION_ALE1D,  i.e.,  it  requires  a  3D 
ALE formulation. 
If  a  title  is  not  defined  LS-DYNA  will  automatically  create  an  internal  title  for  this 
coupling definition.  
Title Card.  Additional card for TITLE and ID keyword options. 
Title 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
COUPID 
Type 
I 
TITLE 
A70 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SLAVE  MASTER 
SSTYP 
MSTYP 
MCOUP 
Type 
I 
I 
Default 
none 
none 
I 
0 
I 
0 
I
Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
START 
END 
PFORM 
PFAC 
FRCMIN 
Type 
Default 
F 
0 
F 
1.0E10 
I 
0 
F 
0.1 
F 
0.5 
  VARIABLE   
COUPID 
DESCRIPTION
Coupling  (card)  ID  number  (I10).    If  not  defined,  LSDYNA  will
assign  an  internal  coupling  ID  based  on the  order of  appearance
in the input deck. 
TITLE 
A description of this coupling definition (A70). 
SLAVE 
Slave  set  ID  defining  a  part,  part  set  or  segment  set  ID  of  the 
Lagrangian or slave structure .  See Remark 1.   
MASTER 
Master set ID defining a part or part set ID of the ALE or master 
solid elements . 
SSTYP 
Slave set type of “SLAVE”: 
EQ.0: part set ID (PSID). 
EQ.1: part ID (PID). 
EQ.2: segment set ID (SGSID). 
EQ.3: node set ID (NSID). 
MSTYP 
Master set type of “MASTER”: 
EQ.0: part set ID (PSID). 
EQ.1: part ID (PID). 
MCOUP 
Multi-material option . 
EQ.0: couple with all multi-material groups, 
LT.0:  MCOUP must be an integer.  –MCOUP refers to a set ID 
of an ALE multi-material groups defined in *SET_MUL-
TI-MATERIAL_GROUP. 
START 
Start time for coupling.
VARIABLE   
DESCRIPTION
END 
End time for coupling. 
PFORM 
Penalty stiffness formulations. 
EQ.0: mass based penalty stiffness.  
EQ.1: bulk modulus based penalty stiffness. 
EQ.2: penalty stiffness is determined by the user-provided load 
curve between penetration and penalty pressure. 
Penalty stiffness factor (PFORM = 0 or 1) for scaling the estimated 
stiffness  of  the  interacting  (coupling)  system  or  Load  Curve  ID
(PFORM = 2). 
Only  to  be  used  with  nonzero  MCOUP.    Minimum  volume
fraction  of  the  fluid  materials  included  in  the  list  of  AMMGs  to
activate coupling.  Default value is 0.5. 
PFAC 
FRCMIN 
Remarks: 
When  MCOUP  is  a  negative  integer,  say  for  example  MCOUP = -123,  then  an  ALE 
multi-material  set-ID  (AMMSID)  of  123  must  exist.    This  is  an  ID  defined  by  a  *SET_-
MULTI-MATERIAL_GROUP_LIST card.
*ALE 
Purpose:    This  command  serves  as  a  simplified  constraint  type  coupling  method 
between ALE fluids and a Lagrange rigid body. 
In  certain  FSI  simulations  structure  deformation  is  either  small  or  not  of  the  interest.  
Often times these structures are modeled as rigid bodies to shorten the simulation time 
and reduce the complexity.  For such kind of problems, a full scale ALE/FSI simulation 
is  costly  in  both  simulation  time  and  memory.    This  keyword  provides  a  light-weight 
alternative FSI method for systems with minimal structural response. 
It  has  a  similar  input  format  to  *ALE_ESSENTIAL_BOUNDARY  and  maybe  regarded 
as being an extension of the essential boundary feature.  The documentation for *ALE_-
ESSENTIAL_BOUNDARY_BODY applies, in large part, to this card also. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IPID 
NSID 
Type 
I 
I 
Default 
none 
none 
ALE Coupling Interfaces Cards.  Include one card for each part, part set or segment to 
define ALE coupling interface.  This input ends at the next keyword (“*”) card. 
  Card 2 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
IDTYPE 
ICTYPE 
IEXCL 
Type 
I 
I 
Default 
none 
none 
I 
1 
I 
none 
  VARIABLE   
DESCRIPTION
IPID 
NSID 
Rigid body part ID. 
Node set ID defining ALE boundary nodes to follow Rigid body
motion.
VARIABLE   
DESCRIPTION
ID 
Set  ID  defining  a  part,  part  set  or  segment  set  ID  of  the  ALE
coupling interface.  
IDTYPE 
Type of set ID: 
EQ.0: part set ID (PSID). 
EQ.1: part ID (PID). 
EQ.2: segment set ID (SGSID). 
ICTYPE 
Constraint type: 
EQ.1: No flow through all directions. 
EQ.2: No flow through normal direction.  (slip condition) 
IEXCL 
Segment  Set  ID  to  be  excluded  from  applying  ALE  essential
boundary condition.  For example, inlet/outlet segments.  
Remarks: 
For  ICTYPE = 2,  the  constrained  direction(s)  at  each  surface  node  comes  in  part  from 
knowing  whether  the  node  is  a  surface  node,  an  edge  node,  or  a  corner  node.    If  the 
ALE mesh boundary is identified by part(s) (IDTYPE = 0/1), edge and corner nodes are 
automatically  detected  during  the  segment  generation  process. 
  However,  this 
automatic  detection  is  not  foolproof  for  complicated  geometries.    Identifying  the  ALE 
mesh boundary using segment sets (IDTYPE = 2) is generally preferred for complicated 
geometries  in  order  to  avoid  misidentification  of  edge  and  corner  nodes.    When 
segment  sets  are  used,  the  edge  and  corner  nodes  are  identified  by  their  presence  in 
multiple  segment  sets  where  each  segment  set  describes  a  more  or  less  smooth, 
continuous surface.  The intersections of these surfaces are used to identify edge/corner 
nodes.
*ALE 
Purpose:    This  command  applies  and  updates  essential  boundary  conditions  on  ALE 
boundary  surface  nodes.    Updating  the  boundary  conditions  is  important  if  the  ALE 
mesh moves according to *ALE_REFERENCE_SYSTEM_GROUP.  If the mesh does not 
move, it’s more correct to call it an Eulerian mesh rather than an ALE mesh, but *ALE_-
ESSENTIAL_BOUNDARY can be applied nonetheless. 
Certain  engineering  problems  need  to  constrain  the  flow  along  the  ALE  mesh 
boundary.    A  simple  example  would  be  water  flowing  in  a  curved  tube.    Using  the 
*ALE_ESSENTIAL_BOUNDARY approach, the tube material is not modeled and there 
is  no  force  coupling  between  the  fluid  and  the  tube,  rather  the  interior  volume  of  the 
tube  is  represented  by  the  location  of  the  ALE  mesh.    Defining  SPC  boundary 
conditions  with  a  local  coordinate  system  at  each  ALE  boundary  node  would  be 
extremely  inconvenient  in  such  a  situation.    The  *ALE_ESSENTIAL_BOUNDARY 
command  applies  the  desired  constraints  along  the  ALE  surface  mesh  automatically.  
The  user  only  needs  to  specify  the  part(s)  or  segment  set(s)  corresponding  to the  ALE 
boundary surfaces and the type of constraint desired.   
Boundary  Condition  Cards.    Include  one  card  for  each  part,  part  set  or  segment  on 
which essential boundary conditions are applied.  This input ends at the next keyword 
(“*”) card. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
IDTYPE 
ICTYPE 
IEXCL 
Type 
I 
I 
Default 
none 
none 
I 
1 
I 
none 
  VARIABLE   
DESCRIPTION
ID 
Set ID defining a part, part set or segment set ID of the ALE mesh
boundary.  
IDTYPE 
Type of set ID: 
EQ.0: part set ID (PSID). 
EQ.1: part ID (PID). 
EQ.2: segment set ID (SGSID).
VARIABLE   
DESCRIPTION
ICTYPE 
Constraint type: 
EQ.1: No flow through all directions. 
EQ.2: No flow through normal direction.  (slip condition) 
IEXCL 
Segment  Set  ID  to  be  excluded  from  applying  ALE  essential
boundary condition.  For example, inlet/outlet segments.  
Remarks: 
For  ICTYPE = 2,  the  constrained  direction(s)  at  each  surface  node  comes  in  part  from 
knowing  whether  the  node  is  a  surface  node,  an  edge  node,  or  a  corner  node.    If  the 
ALE  mesh  boundary  is  identified  by  part(s)  (IDTYPE = 0/1),  edge/corner  nodes  are 
automatically  detected  during  the  segment  generation  process. 
  However,  this 
automatic  detection  is  not  foolproof  for  complicated  geometries.    Identifying  the  ALE 
mesh boundary using segment sets (IDTYPE = 2) is generally preferred for complicated 
geometries  in  order  to  avoid  misidentification  of  edge/corner  nodes.    When  segment 
sets  are  used,  the  edge/corner  nodes  are  identified  by  their  presence  in  multiple 
segment  sets  where  each  segment  set  describes  a  more  or  less  smooth,  continuous 
surface.    In  short,  the  junctures  or  intersections  of  these  surfaces  identify  edge/corner 
nodes.
*ALE 
Purpose:    This  card  is  used  to  allow  the  switching  of  an  ALE  multi-material-group  ID 
(AMMGID) if a failure criteria is reached.  If this card is not used and *MAT_VACUUM 
has  a  multi-material  group  in  the  input  deck,  failed  ALE  groups  are  replaced  by  the 
group for *MAT_VACUUM.  
Available options include: 
<BLANK> 
ID 
TITLE 
A title for the card may be input between the 11th and 80th character on the title-ID line.  
The optional title line precedes all other cards for this command. 
The user can explicitly define a title for this coupling. 
Title Card.  Additional card for the ID or TITLE options to keyword. 
Title 
Variable 
1 
ID 
Type 
I10 
2 
3 
4 
5 
6 
7 
8 
TITLE 
A70 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FR_MMG  TO_MMG 
Type 
I 
I 
Default 
none 
none 
  VARIABLE   
FR_MMG 
DESCRIPTION
This  is  the  AMMG-SID  before  the  switch.    The  AMMG-SID 
corresponds to the SID defined under the *SET_MULTI-MATERI-
AL_GROUP_LIST  (SMMGL)  card.    This  SID  points  to  one  or 
more AMMGs.  See Remark 1.
This  is  the  AMMG-SID  after  the  switch.    The  AMMG-SID 
corresponds to the SID defined under the *SET_MULTI-MATERI-
AL_GROUP_LIST card.  This SID points to one or more AMMGs. 
See Remark 1. 
*ALE 
  VARIABLE   
TO_MMG 
Remarks: 
1.  There is a correspondence between the FR_MMG and TO_MMG.  Consider an 
example where: 
a)  The FR_MMG SID points to a SID = 12 (the SID of its SMMGL card is 12, 
and this SID contains AMMG 1 and AMMG 2) 
b)  The TO_MMG points to a SID = 34 (the SID of the SMMGL card is 34, and 
this SID contains AMMG 3 and AMMG 4) 
Then, AMMG 1, if switched, will become AMMG 3, and AMMG 2, if switched, 
will become AMMG 4.
*ALE 
Purpose:    When  a  material  fails,  this  card  is  used  to  switch  the  failed  material  to 
  When  used  with  FRAGTYP = 2,  it  can  be  used  to  model  material 
vacuum. 
fragmentation.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FR_MMG  TO_MMG  FRAGTYP
Type 
I 
I 
I 
Default 
none 
none 
none 
DESCRIPTION
This  is  the  AMMGID  of  the  material  that  just  fails,  before  the
switch.  
This  is  the  AMMGID  of  the  vacuum  that  the  failed  material  is
being switched to.   
Flag  defining  whether  the  failed  material  is  completely  or
partially switched to vacuum .  
EQ.1:  Fully switch; all failed material is switched to vacuum. 
EQ.2:  Partially switch; only the volume expansion from the last
time step is switched to vacuum. 
  VARIABLE   
FR_MMG 
TO_MMG 
FRAGTYP 
Remarks: 
The Lagrange element contains only one material.  Once the failure criterion is met in a 
Lagrange element, the whole element is marked as “failed” and either deleted or kept 
from further element force calculation. 
However,  for  multi-material  ALE  elements,  such  approach  is  not  practical  as  these 
elements  are  occupied  by  multiple  materials.    Failure,  therefore,  cannot  be  adequately 
modeled  at  the  element  level.    Instead  we  convert  the  failed  material  inside  an  ALE 
element to vacuum.  The effect is similar to element deletion in Lagrange simulations.  
The  failed  material,  once  switched  to  vacuum,  is  excluded  from  any  future  element 
force calculation.
1.  Switch  to  Vacuum,  (FRAGTYPE  =  1).    By  default  multi-material  elements 
switch failed materials to vacuum.  This switch involves assigning the full vol-
ume fraction of the failed material, say AMMG 1, in an element to vacuum, say 
AMMG 2. 
FRAGTYP = 1  is  equivalent  to  the  default  treatment.    However,  with  this  card 
the vacuum AMMG can be explicitly specified.  In the case that more than one 
vacuum  AMMG  exist,  it  is  strongly  recommended  to  use  the  FRAGTYP = 1 
approach to eliminate ambiguity.  It is also helpful during post-processing since 
it is possible to see the material interface of the switched material by assigning a 
dedicated vacuum AMMG to the switched material. 
2.  Fragmentation,  (FRAGTYPE  =  2).    FRAGYP  =  2  models  material  fragmenta-
tion.    Note  that  the  FRAGTYP =  1  approach  leads  to  loss  of  mass  and,  conse-
quently, dissipates both momentum and energy.  With FRAGTYP = 2, instead 
of converting the full volume of the failed material to vacuum, LS-DYNA only 
converts the material expansion to vacuum.  This approach conserves mass and, 
therefore, momentum and energy. 
To  illustrate  how  this  fragmentation  model  works,  consider  a  tension  failure 
example.    At  the  time  step  when  the  material  fails,  LS-DYNA  calculates  the 
material  expansion  in  the  current  step  and  converts  this  volume  to  vacuum.  
The stresses and other history variables are left unchanged, so that in the next 
time  step  it  will  again  fail.    The  expansion  in  the  next  time  step  will  be  also 
converted  to  vacuum.    This  process  continues  until  maybe  at  a  later  time  the 
gap stops growing or even starts to close due to compression. 
Example: 
Consider a simple bar extension example: 
FR_MMG:  H5  =  AMMG1  =  Metal bar 
  H6  =  AMMG2  =  Ambient air 
TO_MMG:  H7  =  AMMG3  =  Dummy vacuum part
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
*ALE_FRAGMENTATION 
$   FR_MMG    TO_MMG   FRAGTYP 
         1         3         2 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8
*ALE 
Purpose:  This card provides a coupling method for simulating the interaction between 
a  Lagrangian  material  set  (structure)  and  ALE  material  set  (fluid).    The  nearest  ALE 
nodes  are  projected  onto  the  Lagrangian  structure  surface  at  each  time  step.    This 
method  does  not  conserve  energy,  as  mass  and  momentum  are  transferred  via 
constrained based approach. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LAGSID 
ALESID 
LSIDTYP  ASIDTYP  SMMGID 
ICORREC 
INORM 
I 
0 
3 
I 
0 
4 
I 
0 
5 
I 
0 
6 
I 
0 
7 
8 
Type 
Default 
I 
0 
  Card 2 
1 
I 
0 
2 
Variable 
BIRTH 
DEATH 
Type 
F 
F 
Default 
0.0 
1.E+10 
  VARIABLE   
LAGSID 
DESCRIPTION
A  set  ID  defining  the  Lagrangian  part(s)  for  this  coupling
(structures). 
ALESID 
A set ID defining the ALE part(s) for this coupling (fluids). 
LSIDTYP 
Lagrangian set ID type 
EQ.0: Part set ID (PSID), 
EQ.1: Part ID (PID). 
ASIDTYP 
ALE set ID type 
EQ.0: Part set ID (PSID), 
EQ.1: Part ID (PID).
SMMGID 
*ALE_FSI_PROJECTION 
DESCRIPTION
A set ID referring to a group of one or more ALE-Multi-Material-
Group  (AMMG)  IDs  which  represents  the  ALE  materials
interacting with the Lagrangian structure.  This SMMGID is a set 
ID defined by *SET_MULTI-MATERIAL_GROUP_LIST. 
ICORREC 
Advection error correction method . 
EQ.1: ALE mass is conserved.  Leaked mass is moved, 
EQ.2: ALE mass is almost conserved, 
EQ.3: No  correction  performed  (default). 
is
conserved.    Some  leakage  may  occur.    This  may  be  the
best solution. 
  ALE  mass 
INORM 
Type of coupling. 
EQ.0: Couple in all directions, 
EQ.1: Couple in compression and tension (free sliding), 
EQ.2: Couple  in  compression  only  (free  sliding).    This  choice
requires ICORREC = 3. 
BIRTH 
Start time for coupling. 
DEATH 
End time for coupling. 
Remarks: 
1.  As the ALE nodes are projected onto the closest Lagrangian surface, there may 
be  some  advection  errors  introduced.    These  errors  may  result  in  a  small  ele-
ment mass fraction being present on the “wrong” side of the coupled Lagrangi-
an surface.  There are 3 possible scenarios: 
a)  Mass on the wrong side of the Lagrangian structure may be moved to the 
right side.  This may cause P oscillations.  No leakage will occur. 
b)  Mass on the wrong side is deleted.  Mass on the right side is scaled up to 
compensate for the lost mass.  No leakage will occur. 
c)  Mass on the wrong side is allowed (no correction performed).  Some leak-
age may occur.  This may be the most robust and simplest approach.
Model Summary: 
*ALE 
H1 = AMMG1 = background air mesh 
H2 = AMMG1 = background air mesh 
S3 = cylinder containing AMMG2 
S4 = dummy target cylinder for impact 
The gas inside S3 is AMMG2.  S3 is given an initial velocity and it will impact S4. 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
*ALE_MULTI-MATERIAL_GROUP 
         1         1 
         2         1 
*SET_MULTI-MATERIAL_GROUP_LIST 
        22 
         2 
*ALE_FSI_PROJECTION 
$   LAGSID    ALESID   LSIDTYP   ASIDTYP    SMMGID   ICORREC     INORM 
         3         1         1         1        22         3         2 
$    BIRTH     DEATH 
       0.0      20.0 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8
*ALE_FSI_SWITCH_MMG 
Purpose:    This  card  is  used  to  allow  the  switching  of  an  ALE  multi-material-group  ID 
(AMMGID) of a fluid as that fluid passes across a monitoring surface.  This monitoring 
surface  may  be  a  Lagrangian  shell  structure,  or  a  segment  set.    It  does  not  have  to  be 
included in the slave set of the coupling card: *CONSTRAINED_LAGRANGE_IN_SOL-
ID. However, at least one coupling card must be present in the model. 
Available options include: 
<BLANK> 
ID 
TITLE 
An ID number (up to 8 digits) may be defined for this switch command in the first 10-
character space.  A title for the card may be input between the 11th and 80th character on 
the title-ID line.  The optional title line precedes all other cards for this command. 
The user can explicitly define a title for this coupling. 
Title Card.  Additional card for the Title or ID keyword options.  
Title 
Variable 
1 
ID 
Type 
I10 
2 
3 
4 
5 
6 
7 
8 
TITLE 
A70 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
STYPE 
NQUAD 
XOFF 
BTIME 
DTIME 
NFREQ 
NFOLD 
Type 
I 
Default 
none 
I 
0 
I 
1 
F 
F 
F 
0.0 
0.0 
1.0E20 
I 
1 
I
Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FR_MMG  TO_MMG 
XLEN 
Type 
I 
I 
F 
Default 
none 
none 
0.0 
  VARIABLE   
SID 
DESCRIPTION
A  set  ID  defining  a  monitoring  surface  over  which  an  ALE  fluid
flows across, and its ALE multi-material-group-ID (AMMGID) is 
switched.    The  monitoring  surface  may  be  a  Lagrangian  shell 
structure, or a segment set.  This surface, if Lagrangian, does not
have to be included in the coupling definition . 
STYPE 
Set ID type of the above SID. 
EQ.0: Part set ID (PSID) (default). 
EQ.1: Part ID (PID). 
EQ.2: Segment set ID (SGSID). 
NQUAD 
XOFF 
The  number  of  flow-sensor  points  to  be  distributed  over  each 
monitoring  surface/segment.    There  should  be  enough  sensor
points  distributed  to  monitor  the  flow  in  each  ALE  element
intersected by this monitoring surface (default = 1, see remark 3).  
An  offset  distance  away  from  the  monitoring  surface,  beyond
which the AMMGID switching occurs.  The direction of XOFF is
defined  by  the  normal  vector  of  the  monitoring  segment.    This
offset  distance,  in  general,  should  be  at  least  2  ALE  element
widths  away  from,  and  beyond  the  monitoring 
interface
(default = 0.0). 
BTIME 
Start time for the AMMGID switch to be activated (default = 0.0).
DTIME 
Ending time for the AMMGID switch (default = 1.0E20). 
NFREQ 
Number  of  computational  cycles  between  ALE  switch  check
(default = 1).
Flag for checking folding logic (default = 0, ⇒ off).  If NFOLD = 1 
(⇒ on), then LS-DYNA will check if the monitoring segment is in
the  fold,  applicable  to  airbag.    If  the  monitoring  segment  is  still
located  within  a  folded  (shell)  region,  then  no  switching  is 
allowed yet until it has unfolded. 
This  is  the  AMMG-SID  before  the  switch.    The  AMMG-SID 
corresponds to the SID defined under the *SET_MULTI-MATERI-
AL_GROUP_LIST  (SMMGL)  card.    This  SID  points  to  one  or 
more AMMGs.  See Remark 1. 
This  is  the  AMMG-SID  after  the  switch.    The  AMMG-SID 
corresponds to the SID defined under the *SET_MULTI-MATERI-
AL_GROUP_LIST card.  This SID points to one or more AMMGs. 
See Remark 1. 
This is an absolute distance for distributing the flow sensor points 
over the ALE elements.  To make sure that at least 1 sensor point,
defined  on  each  Lagrangian  segment,  is  present  in  each  ALE
element to track the flow of an AMMG, XLEN may be estimated
as  roughly  half  the  length  of  the  smallest  ALE  element  in  the 
mesh.  See Remark 3.   
*ALE 
  VARIABLE   
NFOLD 
FR_MMG 
TO_MMG 
XLEN 
Remarks: 
1.  There is a correspondence between the FR_MMG and TO_MMG.  Consider an 
example where: 
a)  The FR_MMG SID points to a SID = 12 (the SID of its SMMGL card is 12, 
and this SID contains AMMG 1 and AMMG 2) 
b)  The TO_MMG points to a SID = 34 (the SID of the SMMGL card is 34, and 
this SID contains AMMG 3 and AMMG 4) 
Then, AMMG 1, if switched, will become AMMG 3, and AMMG 2, if switched, 
will become AMMG 4. 
2.  The ID option must be activated if the parameter SWID is used in the *DATA-
BAS_FSI  card.    Then  the  accumulated  mass  of  an  AMMG  that  goes  through  a 
tracking  surface,  and  being  switched,  will  be  reported  via  the  parameter 
“mout”  in  the  “dbfsi”  ASCII  output  file  (or  equivalently  the  “POROSITY”  pa-
rameter inside LS-PrePost ASCII plotting option).
3.  When  both  NQUAD  and  XLEN  are  defined,  whichever  gives  smaller  sensor-
point  interval  distance  will  be  used.    XLEN  may  give  better  control  as  in  the 
case  of  a  null  shell  acting  as  the  monitoring  surface.    As  this  null  shell  is 
stretched,  NQUAD  distribution  of  sensor-points  may  not  be  adequate,  but 
XLEN would be. 
4.  The  monitoring  surface  does  not  have  to  be  included  in  the  slave  set  of  the 
coupling  card.    However,  at  least  one  coupling  card  must  be  present  in  the 
model.    The  monitoring  segment  set  can  be  made  up  of  Lagrangian  or  ALE 
nodes. 
Example: 
Consider a simple airbag model with 3 part IDs: 
H25 (AMMG1)  =  Inflator gas injected into the airbag. 
H24 (AMMG2)  =  Air outside the airbag (background mesh). 
H26 (AMMG3)  =  Dummy AMMG of inflator gas after it passes through a vent hole.
S9  =  A Lagrangian shell part representing a vent hole. 
S1  =  A Lagrangian shell part representing the top half of an airbag. 
S2  =  A Lagrangian shell part representing the bottom half of an airbag.
The inflator gas inside the airbag is distinguished from the inflator gas that has passed 
through  the  monitoring  surface  (vent  hole)  to  the  outside  of  the  airbag  by  assigning 
different ALE multi-material group set ID to each.  The dummy fluid part (H26) should 
have the same material and EOS model IDs as the before-switched fluid (H25). 
TO_MMG = 125  
⇒ AMMGID (before switch) = *SET_MULTI-MATERIAL_GROUP_LIST(125) = 1  
⇒ PART = PART(AMMGID1) = H25  
FR_MMG = 126  
⇒ AMMGID (before switch) = *SET_MULTI-MATERIAL_GROUP_LIST(126) = 3  
⇒ PART = PART(AMMGID3) = H26 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
*ALE_MULTI-MATERIAL_GROUP 
        25         1 
        24         1 
        26         1 
*DATABASE_FSI 
$     TOUT                                  [STYPE: 0=PSID ; 1=PID ; 2=SGSID] 
    0.1000 
$ DBFSI_ID       SID     STYPE  AMMGSWID  LDCONVID 
         1         1         1 
         2         2         1   
         3         9         1     90000
*SET_MULTI-MATERIAL_GROUP_LIST 
       125 
         1 
*SET_MULTI-MATERIAL_GROUP_LIST 
       126 
         3 
*ALE_FSI_SWITCH_MMG_ID 
     90000 
$      SID   SIDTYPE     NQUAD      XOFF     BTIME     DTIME     NFREQ      FOLD 
         9         1         3     -20.0       5.0       0.0         1         1 
$   Fr_MMG    To_MMG     XCLEN 
       125       126        5. 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
Note: 
1.  The *DATABASE_FSI card tracks 3 surface entities: (a) top half of an airbag, (b) 
bottom  half  of  an  airbag,  and  (c)  the  vent  hole  monitoring  surface  where  the 
AMMGID of the inflator gas is switched. 
2.  The amount of mass passing through the vent hole during the switch is output 
to a parameter called “pleak” in a “dbfsi” ASCII file.  See *DATABASE_FSI. 
3.  The *ALE_FSI_SWITCH_MMG_ID card track any flow across S9 and switch the 
AMMGSID from 125 (AMMG 1) to 126 (AMMG 3).
*ALE 
Purpose:    Output  the  ALE  coupling  forces  from  *CONSTRAINED_LAGRANGE_IN_-
SOLID, CTYPE = 4 in keyword format, so they may be applied directly in another run. 
  Card 1 
Variable 
1 
DT 
2 
3 
4 
5 
6 
7 
8 
NSID 
IOPT 
Type 
I 
I 
Default 
none 
none 
I 
0 
  VARIABLE   
DESCRIPTION
DT 
NSID 
IOPT 
Output intervals 
Node Set ID.  See *SET_NODE. 
Options to map the coupling data between 2 runs:  
EQ.0: The keyword alefsiloadnode.k  is created 
at the end of the run by LS-DYNA. 
EQ.1: A  database  of  coupling  forces  is  dumped  without  the
conversion  in  keyword  file  at  the  end  of  the  run  .    The  database  can  be    treated  by  a  program
(alefsiloadnode.exe) to write alefsiloadnode.k. 
EQ.2: The database of coupling forces created by IOPT = 1  is read back.  The structure meshes should be
identical.  The forces are directly applied the nodes with-
out using *LOAD_NODE.  The parameters DT and NSID 
are not read. 
EQ.3: A  database  of  coupling  accelerations  is  dumped  at  the
end of the run . 
EQ.4: The  database  of  coupling  accelerations  created  by
IOPT = 3    is  read  back.    The  structure
meshes  can  be  different.    The  accelerations  are  interpo-
lated  at  the  nodes  provided  by  NSID.    The  parameters
DT and NSID are read.
*ALE_FSI_TO_LOAD_NODE 
1.  The  name  of  the  output  keyword  file  is  alefsiloadnode.k.    For  each  node,  this 
file  contains  three  *LOAD_NODE  for  each  global  direction  and  three  *DE-
FINE_CURVE for the coupling force histories. 
2.  The  name  of  the  database  is  alefsi2ldnd.tmp  (or  alefsi2ldnd.tmp00…  in  MPP).  
It should be in the directory of the 2nd run for IOPT = 2.  The database lists the 
coupling forces by node.  The structure meshes (and their MPP decomposition) 
for the IOPT = 1 and IOPT = 2 runs should be the same. 
3.  The  names  of  the  databases  are  alefsi2ldnd.tmp  (or  alefsi2ldnd.tmp00…  in 
MPP) and alefsi2lndndx.tmp.  They should be in the directory of the 2nd run for 
IOPT = 4.    The  file  alefsi2ldnd.tmp  lists  the  coupling  accelerations  by  node 
file 
(coupling  acceleration = coupling 
alefsi2lndndx.tmp  lists  the  initial  nodal  coordinates  and  coupling  segment 
connectivities  .    The  structure  meshes  for  the  IOPT = 3  and  IOPT = 4  runs  can  be 
different.  The IOPT = 3 initial geometry stored in alefsi2lndndx.tmp is used to 
interpolate  the  coupling  accelerations  (saved  in  alefsi2ldnd.tmp)  at  the  nodes 
provided by NSID.  For the interpolation to work, these nodes should be within 
the IOPT = 3 coupling segment initial locations.
force  /  nodal  mass). 
  The
*ALE_MULTI-MATERIAL_GROUP 
*ALE_MULTI-MATERIAL_GROUP 
*ALE 
Purpose:  This command defines the appropriate ALE material groupings for interface 
reconstruction when two or more ALE Multi-Material Groups (AMMG) are present in a 
model.    This  card  is  required  when  ELFORM = 11  in  the  *SECTION_SOLID  card  or 
when  ALEFORM = 11  in  *SECTION_ALE1D  or  *SECTION_ALE2D.    Each  data  line 
represents one ALE multi-material group (AMMG), with the first line referring to AM-
MGID  1,  second  line  AMMGID  2,  etc.    Each  AMMG  represents  one  unique  “fluid” 
which may undergo interaction with any Lagrangian structure in the model.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
IDTYPE 
Type 
I 
Default 
none 
I 
0 
Remarks 
1 
  VARIABLE   
DESCRIPTION
SID 
Set ID. 
IDTYPE 
Set type: 
EQ.0: Part set, 
EQ.1: Part. 
Remarks: 
1.  When ELFORM = 12 in the *SECTION_SOLID card (single material and void), 
this card should not be used.  In one model, ELFORM = 12 cannot be used to-
gether  with  ELFORM = 11.    If  possible,  it  is  recommended  that  ELFORM = 11 
be  used  as  it  is  the  most  robust  and  versatile  formulation  for  treating  multi-
material ALE parts. 
2.  Each  AMMG  is  automatically  assigned  an  ID  (AMMGID),  and  consists  of  one 
or  more  PART  ID’s.    The  interface  of  each  AMMGID  is  reconstructed  as  it 
evolves  dynamically.    Each  AMMGID  is  represented  by  one  material  contour 
color in LS-PrePost.
Physical
Material 3
(PID 44)
Physical
Material 3
(PID 55)
Physical
Material 3
(PID 66)
Physical
Material 4
(PID 77)
Physical
Material 1
(PID 11)
Physical
Material 2
(PID 22)
Physical
Material 2
(PID 33)
Figure 4-1.  Schematic illustration of Example 1. 
3.  The  maximum  number  of  AMMGIDs  allowed  has  been  increased  to  20.  
However,  there  may  be  2,  at  most  3,  AMMGs  inside  an  ALE  element  at  any-
time.    If  there  are  more  than  3  AMMGs  inside  any  1  ALE  element,  the  ALE 
mesh  needs  refinement.    Better  accuracy  is  obtained  with  2  AMMGs  in  mixed 
elements. 
4.  To plot these AMMGIDs in LS-PrePost: 
[FCOMP] ⇒ [MISC] ⇒ [VOLUME FRACTION OF AMMGID #] ⇒ [APPLY] 
(Note:  Contour definitions maybe different for gas mixture application) 
5. 
It is very important to distinguish among the  
a)  Physical materials,  
b)  PART IDs, and  
c)  AMMGIDs. 
A  *PART  may  be  any  mesh  component.    In  ALE  formulation,  it  is  simply  a 
geometric entity and a time = 0 concept.   This means a *PART  may be a mesh 
region that can be filled with one or more AMMGIDs at time zero, via a volume 
filling  command  (*INITIAL_VOLUME_FRACTION_GEOMETRY).    An  AM-
MGID  represents  a  physical  material  group  which  is  treated  as  one  material
entity  (represented  by  1  material  color  contour  in  LS-PrePost  plotting).  
AMMGID  is  used  in  dealing  with  multiple  ALE  or  Eulerian  materials.    For 
example, it can be used to specify a master ALE group in a coupling card. 
Example 1: 
Consider  a  purely  Eulerian  model  containing  3  containers  containing  2  different 
physical materials (fluids 1 and 2).  All surrounded by the background material (maybe 
air).    The  containers  are  made  of  the  same  material,  say,  metal.    Assume  that  these 
containers explode and spill the fluids.  We want to track the flow and possibly mixing 
of the various materials.  Note that all 7 parts have ELFORM = 11 in their *SECTION_-
SOLID cards.  So we have total of 7 PIDs, but only 4 different physical materials.  See 
Figure 4-1. 
Approach 1:  If we want to track only the interfaces of the physical materials. 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
*SET_PART 
         1 
        11 
*SET_PART 
         2 
        22        33 
*SET_PART 
         3 
        44        55        66 
*SET_PART 
         4 
        77 
*ALE_MULTI-MATERIAL_GROUP 
         1         0   ←   1st line = 1st AMMG ⇒AMMGID = 1 
         2         0   ←  2nd line = 2nd AMMG ⇒AMMGID = 2 
         3         0   ←  3rd line = 3rd AMMG ⇒AMMGID = 3 
         4         0   ←  4th line = 4th AMMG ⇒AMMGID = 4 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
With this approach, we define only 4 AMMGs (NALEGP = 4).  So in LS-PrePost, when 
plotting  the  material-group  (history  variable)  contours,  we  will  see  4  colors,  one  for 
each material group.  One implication is that when the fluids from part 22 and part 33 
flow  into  the  same  element,  they  will  coalesce  and  no  boundary  distinction  between 
them  is  maintained  subsequently.    While  this  may  be  acceptable  for  fluids  at  similar 
thermodynamic  states,  this  may  not  be  intuitive  for  solids.    For  example,  if  the  solid 
container  materials  from  parts  44,  55  and  66  flow  into  one  element,  they  will  coalesce 
“like a single fluid”, and no interfaces among them are tracked.  If this is undesirable, 
an alternate approach may be taken.  It is presented next.
Approach 2:  If we want to reconstruct as many interfaces as necessary, in this case, we 
follow the interface of each part. 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
*ALE_MULTI-MATERIAL_GROUP 
         1         1   ←   1st line = 1st AMMG ⇒AMMGID = 1 
         2         1   ←  2nd line = 2nd AMMG ⇒AMMGID = 2 
         3         1   ←  3rd line = 3rd AMMG ⇒AMMGID = 3 
         4         1   ←  4th line = 4th AMMG ⇒AMMGID = 4 
         5         1   ←  4th line = 5th AMMG ⇒AMMGID = 5 
         6         1   ←  4th line = 6th AMMG ⇒AMMGID = 6 
         7         1   ←  4th line = 7th AMMG ⇒AMMGID = 7 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
There are 7 AMMGs in this case (NALEGP = 7).  This will involve more computational 
cost  for  the  additional  tracking.    Realistically,  accuracy  will  be  significantly  reduced  if 
there  are  more  than  3  or  4  materials  in  any  one  element.    In  that  case,  higher  mesh 
resolution may be required. 
Example 2: 
Oil 
Water 
Air 
Group 1 
Group 2 
Group 3 
Part IDs 1 and 2 
Part ID 3 
Part IDs 5, 6, and 7 
The  above  example  defines  a  mixture  of  three  groups  of  materials  (or  “fluids”),  oil, 
water  and  air,  that  is,  the  number  of  ALE  multi-material  groups  (AMMGs) 
NALEGP = 3. 
The first group contains two parts (materials), part ID's 1 and 2. 
The second group contains one part (material), part ID 3. 
The third group contains three parts (materials), part ID's 5, 6 and 7.
*ALE 
Purpose:    This  command  defines  a  motion  and/or  a  deformation  prescribed  for  a 
geometric  entity,  where  a  geometric  entity  may  be  any  part,  part  set,  node  set,  or 
segment  set.    The  motion  or  deformation  is  completely  defined  by  the  12  parameters 
shown  in  the  equation  below.    These  12  parameters  are  defined  in  terms  of  12  load 
curves.  This command is required only when PRTYPE = 3 in the *ALE_REFERENCE_-
SYSTEM_GROUP command. 
2 
3 
4 
5 
6 
7 
8 
  Card 1 
Variable 
1 
ID 
Type 
I 
Default 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID1 
LCID2 
LCID3 
LCID4 
LCID5 
LCID6 
LCID7 
LCID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID9 
LCID10 
LCID11 
LCID12 
Type 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
ID 
Curve group ID. 
LCID1, …, LCID12 
Load curve IDs.
*ALE_REFERENCE_SYSTEM_CURVE 
1.  The velocity of a node at coordinate (𝑥, 𝑦, 𝑧) is defined as: 
{⎧𝑥̇
}⎫
𝑦̇
𝑧̇⎭}⎬
⎩{⎨
=
{⎧𝑓1
}⎫
𝑓5
𝑓9⎭}⎬
⎩{⎨
+
𝑓2
⎡
𝑓6
⎢
𝑓10
⎣
𝑓3
𝑓7
𝑓11
𝑓4
⎤
𝑓8
⎥
𝑓12⎦
{⎧𝑥 − XC
}⎫
𝑦 − YC
𝑧 − ZC⎭}⎬
⎩{⎨
where 𝑓1(𝑡) is the value of load curve LCID1 at time 𝑡, 𝑓2(𝑡) is the value of load 
curve LCID2 at time 𝑡 and so on.  The functions 𝑓1(𝑡), 𝑓5(𝑡), and 𝑓9(𝑡) respectively 
correspond to the translation components in global 𝑥, 𝑦, and 𝑧 direction, while 
the functions 𝑓2(𝑡), 𝑓7(𝑡),  and 𝑓12(𝑡) correspond to and expansion or contraction 
along the 𝑥, 𝑦, and 𝑧 axes. 
The  parameters  XC,  YC  and  ZC  from  the  second  data  card  of  *ALE_REFER-
ENCE_SYSTEM_GROUP  define  the  center  of  rotation  and  expansion  of  the 
mesh.    If  the  mesh  translates,  the  center  position  is  updated  with  𝑓1(𝑡), 𝑓5(𝑡), 
and 𝑓9(𝑡). 
If    LCID8,  LCID10,  LCID3  are  equal  to  −1,  their  corresponding  values  𝑓8(𝑡), 
𝑓10(𝑡), and 𝑓3(𝑡) will be equal to −𝑓11(𝑡), −𝑓4(𝑡), and −𝑓6(𝑡) so as to make a skew 
symmetric matrix thereby inducing a rigid rotation of the mesh about the axis 𝐯 
defined by the triple, 
𝐯 = (𝑓11(𝑡), 𝑓4(𝑡), 𝑓6(𝑡)) 
Example: 
Consider  a  motion  that  consists  of  translation  in  the  x  and  y  direction  only.    Thus 
only 𝑓1(𝑡) and 𝑓5(𝑡) are required.  Hence only 2 load curve ID’s need be defined: 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 
*ALE_REFERENCE_SYSTEM_GROUP 
$      SID     STYPE     PRTYP      PRID    BCTRAN     BCEXP     BCROT    ICOORD 
         1         0         3        11         0         7         0 
$       XC        YC        ZC    EXPLIM 
         0         0         0         0  
*ALE_REFERENCE_SYSTEM_CURVE 
$ CURVESID 
        11 
$    LCID1     LCID2     LCID3     LCID4     LCID5     LCID6     LCID7    LCID8      
       111         0         0         0       222         0         0        0 
$    LCID9    LCID10    LCID11    LCID12  
         0         0         0         0 
*DEFINE_CURVE 
$     lcid      sidr       sfa       sfo      offa      offo    dattyp     
       111          
$                 a1                  o1                   
                0.00                 5.0 
                0.15                 4.0 
*DEFINE_CURVE 
$     lcid      sidr       sfa       sfo      offa      offo    dattyp     
       222          
$                 a1                  o1                   
                0.00                -1.0
0.15                -5.0 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8
*ALE_REFERENCE_SYSTEM_GROUP 
Purpose:  This card is used to associate a geometric entity to a reference system type.  A 
geometric  entity  may  be  any  part,  part  set,  node  set,  or  segment  set  of  a  model  (or  a 
collection  of  meshes).    A  reference  system  type  refers  to  the  possible  transformation 
allowed for a geometric entity (or mesh).  This command defines the type of reference 
system  or  transformation  that  a  geometric  entity  undergoes.    In  other  words,  it 
prescribes how certain mesh can translate, rotate, expand, contract, or be fixed in space, 
etc. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
STYPE 
PRTYPE 
PRID 
BCTRAN 
BCEXP 
BCROT 
ICR/NID 
Type 
I 
Default 
none 
  Card 2 
Variable 
1 
XC 
Type 
F 
I 
0 
2 
YC 
F 
I 
0 
3 
ZC 
F 
I 
0 
4 
I 
0 
5 
I 
0 
6 
I 
0 
7 
I 
0 
8 
EXPLIM 
EFAC 
FRCPAD 
IEXPND 
F 
F 
F 
0.1 
I 
0 
Default 
0.0 
0.0 
0.0 
inf. 
0.0 
Remaining cards are optional.† 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IPIDXCL 
IPIDTYP 
Type 
Default 
I 
0 
I
VARIABLE   
DESCRIPTION
SID 
Set ID. 
STYPE 
Set type: 
EQ.0: part set, 
EQ.1: part, 
EQ.2: node set, 
EQ.3: segment set. 
PRTYPE 
Reference system type : 
EQ.0: Eulerian, 
EQ.1: Lagrangian, 
EQ.2: Normal ALE mesh smoothing, 
EQ.3: Prescribed motion following load curves, see *ALE_REF-
ERENCE_SYSTEM_CURVE, 
EQ.4: Automatic  mesh  motion  following  mass  weighted
average velocity in ALE mesh, 
EQ.5: Automatic  mesh  motion  following  a  local  coordinate
system  defined  by  three  user  defined  nodes,  see  *ALE_-
REFERENCE_SYSTEM_NODE, 
EQ.6: Switching  in  time  between  different  reference  system 
types, see *ALE_REFERENCE_SYSTEM_SWITCH, 
EQ.7: Automatic  mesh  expansion  in  order  to  enclose  up  to
twelve user defined nodes, see *ALE_REFERENCE_SYS-
TEM_NODE. 
EQ.8: Mesh  smoothing  option  for  shock  waves,  where  the 
element  grid  contracts  in  the vicinity  of  the  shock  front:
this  may  be  referred  to  as  the  Delayed-ALE  option.    It 
controls  how  much  the  mesh  is  to  be  moved  during  the
remap step.  This option requires the definition of the 5th
parameter  in  the  2nd  card,  EFAC;  see  below  for  defini-
tion. 
EQ.9: Allowing the ALE mesh(es) to: 
1.  Translate  and/or  rotate  to  follow  a  local  Lagrangian
reference  coordinate  system 
*ALE_REFER-
ENCE_SYSTEM_NODE  card  ID  is  defined  by  the  BC-
TRAN parameter) 
(whose
VARIABLE   
DESCRIPTION
2.  Expand  or  contract  to  enclose  a  Lagrangian  part-set  ID 
defined by the PRID parameter. 
3.  Has  a  Lagrangian  node  ID  be  defined  by  the  ICR/NID
parameter to be the center of the ALE mesh expansion. 
PRID 
A  parameter  giving  additional  information  depending  on  the
reference system (PRTYPE) choice: 
PRTYPE.EQ.3: PRID  defines  a  load  curve  group  ID  specifying
an  *ALE_REFERENCE_SYSTEM_CURVE  card 
for  mesh  translation.    This  defines  up  to  12
curves  which  prescribe  the  motion  of  the  sys-
tem. 
PRTYPE.EQ.4: PRID  defines  a  node  set  ID  (*SET_NODE),  for 
which  a  mass  average  velocity  is  computed.
This velocity controls the mesh motion. 
PRTYPE.EQ.5: PRID  defines  a  node  group  ID  specifying  an
*ALE_REFERENCE_SYSTEM_NODE  card,  via 
which,  three  nodes  forming  a  local  coordinate 
system are defined. 
PRTYPE.EQ.6: PRID  defines  a  switch  list  ID  specifying  an
*ALE_REFERENCE_SYSTEM_SWITCH 
card. 
This defines the switch times and the reference
system  choices  for  each  time  interval  between
the switches. 
PRTYPE.EQ.7: PRID  defines  a  node  group  ID  specifying  an
*ALE_REFERENCE_SYSTEM_NODE  card.    Up 
to 12 nodes in space forming a region to be en-
veloped by the ALE mesh are defined. 
PRTYPE.EQ.9: PRID  defines  a  Lagrangian  part  set  ID  (PSID)
defining the Lagrangian part(s) whose range of 
motion is to be enveloped by the ALE mesh(es).
This is useful for airbag modeling. 
If PRTYPE.EQ.4 or PRTYPE.EQ.5, then 
BCTRAN 
BCTRAN is a translational constraint (Remark 3). 
EQ.0:  no constraints, 
EQ.1:  constrained 𝑥 translation,
VARIABLE   
DESCRIPTION
EQ.2:  constrained 𝑦 translation, 
EQ.3:  constrained 𝑧 translation, 
EQ.4:  constrained 𝑥 and 𝑦 translation, 
EQ.5:  constrained 𝑦 and 𝑧 translation, 
EQ.6:  constrained 𝑧 and 𝑥 translation, 
EQ.7:  constrained 𝑥, 𝑦, and 𝑧 translation. 
Else If PRTYPE.EQ.9, then 
BCTRAN 
BCTRAN  is  a  node  group  ID  from  a  *ALE_REFERENCE_SYS-
TEM_NODE  card  prescribing  a  local  coordinate  system  (3  node
IDs) whose motion is to be followed by the ALE mesh(es). 
Else 
BCTRAN 
Ignored 
End if 
BCEXP 
For  PRTYPE = 4  &  7  BCTRAN  is  an  expansion  constraint,
otherwise it is ignored (Remark 3). 
EQ.0:  no constraints, 
EQ.1:  constrained 𝑥 expansion, 
EQ.2:  constrained 𝑦 expansion, 
EQ.3:  constrained 𝑧 expansion, 
EQ.4:  constrained 𝑥 and 𝑦 expansion, 
EQ.5:  constrained 𝑦 and 𝑧 expansion, 
EQ.6:  constrained 𝑧 and 𝑥 expansion, 
EQ.7:  constrained 𝑥, 𝑦, and 𝑧 expansion. 
BCROT 
BCROT is a rotational constraint (Remark 3).  Otherwise, BCROT 
is ignored. 
EQ.0:  no constraints, 
EQ.1:  constrained 𝑥 rotation, 
EQ.2:  constrained 𝑦 rotation,
VARIABLE   
DESCRIPTION
EQ.3:  constrained 𝑧 rotation, 
EQ.4:  constrained 𝑥 and 𝑦 rotation, 
EQ.5:  constrained 𝑦 and 𝑧 rotation, 
EQ.6:  constrained 𝑧 and 𝑥 rotation, 
EQ.7:  constrained 𝑥, 𝑦, and 𝑧 rotation. 
If PRTYPE.EQ.4 
ICR/(NID) 
ICR  is  a  flag  the  specifies  the  method  LS-DYNA  uses  for 
determining 
the  center  point  for  expansion  and  rotation
(Remark 3). 
EQ.0:  The center is at center of gravity of the ALE mesh. 
EQ.1:  The  center  is  at  (XC,  YC,  ZC),  just  a  point  in  space  (it
does not have to be a defined node) 
Else if PRTYPE.EQ.9 
(ICR)/NID 
NID  sets  the  Lagrangian  node  ID  for  the  node  that  anchors  the
center of ALE mesh expansion (Remark 2). 
End if 
XC, YC, ZC 
EXPLIM 
Center  of  mesh  expansion  and  rotation  for  PRTYPE = 4  and  5, 
otherwise ignored.  See ICR above. 
Limit  ratio  for  mesh  expansion  and  contraction.    Each  Cartesian
direction is treated separately.  The distance between the nodes is
not  allowed  to  increase  by  more  than  a  factor  EXPLIM,  or
decrease  to  less  than  a  factor  1/EXPLIM.    This  flag  applies  only
for PRTYPE = 4, otherwise it is ignored. 
EFAC 
Mesh  remapping  factor  for  PRTYPE = 8  only,  otherwise  it  is 
ignored.    EFAC  is  allowed  to  range  between  0.0  and  1.0.    When
EFAC  approaches  1.0,  the  remapping  approaches  the  Eulerian
behavior. 
The smaller the value of EFAC, the closer the mesh will follow the 
material  flow  in  the  vicinity  of  a  shock  front,  i.e.    approaching
Lagrangian behavior. 
Note  that  excessively small  values  for  EFAC  can  result  in  severe
VARIABLE   
DESCRIPTION
FRCPAD 
mesh distortions as the mesh follows the material flow.  As time 
evolves,  the  mesh  smoothing  behavior  will  approach  that  of  an
Eulerian system. 
For PRTYPE = 9 this is an ALE mesh padding fraction, otherwise
it is ignored. 
FRCPAD is allowed to range from 0.01 to 0.2.  If the characteristic
Lagrange mesh dimension, 𝑑𝐿1, exceeds 
(1 − 2 × FRCPAD) × 𝑑𝐿𝐴, 
where 𝑑𝐿𝐴 is the characteristic length of the ALE mesh,  then the
ALE mesh is expanded so that 
𝑑𝐿𝐴 =
𝑑𝐿1
1 − 2 × FRCPAD
. 
This  provides  an  extra  few  layers  of  ALE  elements  beyond  the
maximum Lagrangian range of motion. 
EQ.0.01:  𝑑𝐿𝐴 =
EQ.0.20:  𝑑𝐿𝐴 =
𝑑𝐿𝐿
⁄
0.98
𝑑𝐿𝐿
⁄
0.60
= 𝑑𝐿𝐿 × 1.020408 
= 𝑑𝐿𝐿 × 1.666667 
IEXPND 
For  PRTYPE = 9  this  is  an  ALE  mesh  expansion  control  flag,
otherwise it is ignored. 
EQ.0:  Both mesh expansion and contraction are allowed. 
EQ.1:  Only mesh expansion is allowed: 
IPIDXCL 
An  ALE  set  ID  to  be  excluded  from  the  expansion  and/or
contraction  only.    Translation  and  rotation  are  allowed.    For
example,  this  may  be  used  to  prevent  the  ALE  mesh  (or  part)  at
the inflator gas inlet region from expanding too much.  High ALE 
mesh resolution is usually required to resolve the high speed flow
of the gas into the airbag via point sources . 
IPIDTYPE 
Set ID type of IPIDXCL: 
EQ.0:  PSID 
EQ.1:  PID
*ALE_REFERENCE_SYSTEM_GROUP 
1.  Required  Associated  Cards.    Some  PRTYP  values  may  require  a  supple-
mental  definition  defined  via  corresponding  PRID.    For  example,  PRTYP = 3 
requires a *ALE_REFERENCE_SYSTEM_CURVE card.  If PRID = n, then in the 
corresponding  *ALE_REFERENCE_SYSTEM_CURVE  card,  ID = n.    Similar 
association applies for any PRTYP (i.e.  3, 5, 6, or 7) which requires a definition 
for its corresponding PRID parameter.  
2.  Mesh  Centering.  For  PRTYPE = 9:  ICR/NID  can  be  useful  to  keep  a  high 
density  ALE  mesh  centered  on  the  region  of  greatest  interest,  (such  as  the  in-
flator orifices region in an airbag model).  For example, in the case of nonsym-
metrical airbag deployment, assuming that the ALE mesh is initially finer near 
the  inlet  orifices,  and  gradually  coarsened  away  from  it.    Defining  an  “anchor 
node”  at  the  center  of  the  orifice  location  will  keep  the  fine  ALE  mesh  region 
centered  on  the  orifice  region.    So  that  this  fine  ALE  mesh  region  will  not  be 
shifted  away  (from  the  point  sources)  during  expansion  and  translation.    The 
ALE mesh can move and expand outward to envelop the Lagrangian airbag in 
such a way that the inlet is well resolved throughout the deployment. 
3.  Additional Constraints.  The table below shows the applicability of the various 
choices  of  PRTYPE.    Simple  deductions  from  the  functional  definitions  of  the 
PRTYPE  choices  will  clarify  the  applications  of  the  various  constraints.    For 
example,  when  PRTYP = 3,  nodal  motion  of  the  ALE  mesh  is  completely  con-
trolled by the 12 curves.  Therefore, no constraints are needed. 
PRTYPE 
ICR/NID 
BCTRAN 
BCROT 
BCEXP 
3 
4 
5 
6 
7 
8 
9 
NO 
YES (ICR) 
NO 
NO 
NO 
NO 
NO 
YES 
YES 
NO 
NO 
NO 
YES (NID) 
YES (NGID) 
NO 
YES 
NO 
NO 
NO 
NO 
NO 
NO 
YES 
NO 
NO 
YES 
NO 
NO 
Example 1: 
Consider  a  bird-strike  model  containing  2  ALE  parts:  a  bird  is  surrounded  by  air  (or 
void).  A part-set ID 1 is defined containing both parts.  To allow for the meshes of these
2  parts  to  move  with  their  combined  mass-weighted-average  velocity,  PRTYPE = 4  is 
used.    Note  that  BCEXP = 7  indicating  mesh  expansion  is  constrained  in  all  global 
directions. 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 
*ALE_REFERENCE_SYSTEM_GROUP 
$      SID     STYPE     PRTYP      PRID    BCTRAN     BCEXP     BCROT    ICOORD 
         1         0         4         0         0         7         0 
$       XC        YC        ZC    EXPLIM 
         0         0         0         0  
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 
Example 2: 
Consider  a  bouncing  ball  model  containing  2  ALE  parts:  a  solid  ball  (PID  1)  is 
surrounded by air or void (PID 2).  A part-set ID 1 is defined containing both parts.  To 
allow  for  the  meshes  of  these  2  parts  to  move  with  2  reference  system  types:  (a)  first, 
they  move  with  their  combined  mass-weighted-average  velocity  between  0.0  and  0.01 
second;  and  subsequently  (between  0.01  and  10.0  seconds)  their  reference  system  is 
switched to (b) an Eulerian system (thus the mesh is fixed in space), a reference system 
“SWITCH”  is  required.    This  is  done  by  setting  PRTYPE = 6.    This  PRTYPE  requires  a 
corresponding *ALE_REFERENCE_SYSTEM_SWITCH card.  Note that PRID = 11 in the 
*ALE_REFERENCE_SYSTEM_GROUP  card  corresponds  to  the  SWITCHID = 11  in 
*ALE_REFERENCE_SYSTEM_SWITCH card. 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
*ALE_REFERENCE_SYSTEM_GROUP 
$      SID     STYPE     PRTYP      PRID    BCTRAN     BCEXP     BCROT    ICOORD 
         1         0         6        11         0         7         7 
$       XC        YC        ZC    EXPLIM   EULFACT SMOOTHVMX 
         0         0         0         0       0.0 
*ALE_REFERENCE_SYSTEM_SWITCH 
$ SWITCHID 
        11 
$       t1        t2        t3        t4        t5        t6        t7  
      0.01      10.0 
$    TYPE1     TYPE2     TYPE3     TYPE4     TYPE5     TYPE6     TYPE7     TYPE8 
         4         0 
$      ID1       ID2       ID3       ID4       ID5       ID6       ID7       ID8 
         0         0         0         0         0         0         0         0 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8
*ALE_REFERENCE_SYSTEM_NODE 
Purpose:    This  command  defines  a  group  of  nodes  that  control  the  motion  of  an  ALE 
mesh.  It is used only when PRTYPE = 5 or 7 in a corresponding *ALE_REFERENCE_-
SYSTEM_GROUP card. 
2 
3 
4 
5 
6 
7 
8 
  Card 1 
Variable 
1 
ID 
Type 
I 
Default 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID1 
NID2 
NID3 
NID4 
NID5 
NID6 
NID7 
NID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID9 
NID10 
NID11 
NID12 
Type 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
ID 
Node group ID for PRTYPE 5 or 7, see *ALE_REFERENCE_SYS-
TEM_GROUP. 
User specified nodes. 
NID1, …, 
NID12
Remarks: 
1.  For  PRTYPE = 5  the  ALE  mesh  is  forced  to  follow  the  motion  of  a  coordinate 
system, which is defined by three nodes (NID1, NID2, NID3).  These nodes are 
located at 𝑥1, 𝑥2 and 𝑥3, respectively.  The axes of the coordinate system,  𝑥′, 𝑦′, 
and 𝑧′, are defined as: 
𝑥′ =
𝑥2 − 𝑥1
|𝑥2 − 𝑥1|
𝑦′ = 𝑧′ × 𝑥′ 
 𝑧′ = 𝑥′ ×
𝑥3 − 𝑥1
∣𝑥′ × (𝑥3 − 𝑥1)∣
Note that 𝑥1 → 𝑥2 is the local 𝑥′axis, 𝑥1 → 𝑥3 is the local 𝑦′ axis and 𝑥′ crosses 𝑦′ 
gives the local 𝑧′ axis.  These 3 nodes are used to locate the reference system at 
any time.  Therefore, their positions relative to each other should be as close to 
an orthogonal system as possible for better transformation accuracy of the ALE 
mesh. 
2.  For PRTYPE = 7, the ALE mesh is forced to move and expand, so as to enclose 
up  to  twelve  user  defined  nodes  (NID1,  …,  NID12).    This  is  a  rarely  used  op-
tion. 
Example 1: 
Consider  modeling  sloshing  of  water  inside  a  rigid  tank.    Assuming  there  are  2  ALE 
parts,  the  water  (PID  1)  and  air  or  void  (PID  2)  contained  inside  a  rigid  (Lagrangian) 
tank (PID 3).  The outer boundary nodes of both ALE parts are merged with the inner 
tank  nodes.    A  part-set  ID  1  is  defined  containing  both  ALE  parts  (PIDs  1  and  2).    To 
allow  for  the  meshes  of  the  2  ALE  parts  to  move  with  the  rigid  Lagrangian  tank, 
PRTYPE = 5 is used.  The motion of the ALE parts then follows 3 reference nodes on the 
rigid tank.  These 3 reference nodes must be defined by a corresponding *ALE_REFER-
ENCE_SYSTEM_NODE card.  In this case the reference nodes have the nodal IDs of 5, 6 
and 7.  Note that PRID = 12 in the  
*ALE_REFERENCE_SYSTEM_GROUP  card  corresponds  to  the  SID = 12  in  the  *ALE_-
REFERENCE_SYSTEM_NODE card.
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 
*ALE_REFERENCE_SYSTEM_GROUP 
$      SID     STYPE     PRTYP      PRID    BCTRAN     BCEXP     BCROT    ICOORD 
         1         0         5        12 
$       XC        YC        ZC    EXPLIM 
         0         0         0         0 
*ALE_REFERENCE_SYSTEM_NODE 
$     NSID 
        12 
$       N1        N2        N3        N4        N5        N6        N7        N8 
         5         6         7 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8
*ALE_REFERENCE_SYSTEM_SWITCH 
Purpose:  The PRTYPE parameter in the *ALE_REFERENCE_SYSTEM_GROUP (ARSG) 
card  allows  many  choices  of  the  reference  system  types  for  any  ALE  geometric  entity.  
This command allows for the time-dependent switches between these different types of 
reference  systems,  i.e.,  switching  to  multiple  PRTYPEs  at  different  times  during  the 
simulation.    This  command  is  required  only  when  PRTYPE = 6  in  ARSG  card.    Please 
see example 2 in the ARSG section. 
2 
3 
4 
5 
6 
7 
8 
  Card 1 
Variable 
1 
ID 
Type 
I 
Default 
none 
  Card 2 
Variable 
1 
T1 
Type 
F 
2 
T2 
F 
3 
T3 
F 
4 
T4 
F 
5 
T5 
F 
6 
T6 
F 
7 
T7 
F 
8 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TYPE1 
TYPE2 
TYPE3 
TYPE4 
TYPE5 
TYPE6 
TYPE7 
TYPE8 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I
Card 4 
1 
Variable 
ID1 
2 
ID2 
3 
ID3 
4 
ID4 
5 
ID5 
6 
ID6 
7 
ID7 
8 
ID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
ID 
Switch list ID, see *ALE_REFERENCE_SYSTEM_GROUP, 
T1, …, T7 
TYPE1, …, 
TYPE8 
Times  for  switching  reference  system  type.    By  default,  the
reference  system  TYPE1  occurs  between  time = 0  and  time = T1, 
and TYPE2 occurs between time = T1 and time = T2, etc. 
Reference system types (also see PRTYPE under ARSG): 
EQ.0: Eulerian, 
EQ.1: Lagrangian, 
EQ.2: Normal ALE mesh smoothing, 
EQ.3: Prescribed motion following load curves, see *ALE_REF-
ERENCE_SYSTEM_CURVE, 
EQ.4: Automatic  mesh  motion  following  mass  weighted
average velocity in ALE mesh, 
EQ.5: Automatic  mesh  motion  following  a  local  coordinate 
system  defined  by  three  user  defined  nodes,  see  *ALE_-
REFERENCE_SYSEM_NODE, 
ID1, …, ID8 
The  corresponding  PRID  parameters  supporting  each  PRTYPE
used during the simulation.   
Remarks: 
1.  The beginning time is assumed to be t = 0, and the starting PRTYPE is TYPE1.  
So at T1, the 1st switching time, PRTYPE is switched from TYPE1 to TYPE2, and 
so forth.  This option can be complex in nature so it is seldom applied.
See *CONTROL_REFINE_ALE. 
*ALE
*ALE_SMOOTHING 
Purpose:    This  smoothing  constraint  keeps  an  ALE  slave  node  at  its  initial  parametric 
location along a line between two other ALE nodes.  If these nodes are not ALE nodes, 
the  slave  node  has  to  follow  their  motion  .    This  constraint  is  active 
during  each  mesh  smoothing  operation.    This  keyword  can  be  used  with  ALE  solids, 
ALE shells and ALE beams. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SNID 
MNID1 
MNID2 
IPRE 
XCO 
YCO 
ZCO 
Type 
I 
I 
I 
Default 
none 
none 
none 
I 
0 
F 
F 
F 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
SNID 
Slave ID, see Figure 4-2. 
GT.0:  SNID is an ALE node, 
EQ.0: the slaves are the nodes of an ALE mesh connected to the
first master nodes (MNID1).  See Remarks 2 and 4. 
LT.0:  |SNID| is a ID of ALE node set.  See Remark 2. 
1st master node
slave node
Figure  4-2.   This  simple  constraint,  which ensures that a  slave node  remains
on  a  straight  line  between  two  master  nodes,  is  sometimes  necessary  during
ALE smoothing. 
2nd master node
VARIABLE   
DESCRIPTION
MNID1 
First master ID. 
GT.0: MNID1 is a node, 
LT.0:  |MNID1| 
is 
if
XCO = YCO = ZCO = 0.0.    Otherwise,  |MNID1|  is  a 
node set ID.  See Remarks 2 and 3. 
segment 
set 
ID 
a 
MNID2 
Second master ID. 
GT.0:  MNID2 is a node, 
EQ.0: the  slave  motion  is  solely  controlled  by  MNID1.    See
Remark 5. 
LT.0:  |MNID2| is a node set ID.  See Remark 2. 
IPRE 
EQ.0: smoothing  constraints  are  performed  after  mesh 
relaxation, 
EQ.1: smoothing  constraints  are  performed  before  mesh
relaxation. 
𝑥-coordinate of constraint vector 
𝑦-coordinate of constraint vector 
𝑧-coordinate of constraint vector 
XCO 
YCO 
ZCO 
Remarks: 
1.  When Master Nodes Are Not ALE Nodes.  If SNID, MNID1 and MNID2 are 
ALE  nodes,  the  positions  of  MNID1  and  MNID2  are  interpolated  to  position 
SNID.    If  MNID1  and MNID2  are  not  ALE  nodes,  the  motions  of MNID1  and 
MNID2 are interpolated to move SNID. 
2.  Node Sets for Constraint Generation.   If  MNID1 is a set, SNID and MNID2 
should be node sets or zeros.  In such a case, the constraints are created during 
the initialization and printed out in a file called alesmoothingenerated.k for the 
user’s convenience.  
3.  Constraint Generation Algorithm.  The constraints for a given master node in 
MNID1  are  generated  by  finding  the  closest  slave  nodes  to  an  axis  passing 
through 
the  constraint  vector 
(XCO,YCO,ZCO) if MNID1 is a node set.  If MNID1 is a segment set, the nor-
the  master  node  and  oriented  by
mals of the segments connected to the master node are averaged to give a direc-
tion to the axis. 
4.  Automatic Identification of Slave Nodes.  If SNID=0, MNID1 should be a set 
of nodes or segments along the boundary of an ALE mesh.  For a given master 
node in MNID1, the constraints are created for all the nodes of the mesh found 
the  closest  to  the  axis  described  previously.    The  search  of  slaves  starts  with 
nodes  of  elements  connected  to  the  master  node  and  stops  when  a  boundary 
node with an element connectivity similar to the master node’s one is reached 
or when a node in the set MNID2 (if defined) is found. 
5.  MNID2  =  0.    If  MNID2=0  and  SNID  is  defined,  MNID1  should  not  be  ALE.  
Otherwise SNID and MNID1 positions would match and the element volumes 
between  them  could  be  zero  or  negative.    Only  SNID  and  MNID1  motion 
should match in such a case.
*ALE 
Purpose:    This  keyword  generates  a  structured  3D  mesh  and  invokes  the  Structured 
ALE (S-ALE) solver.  Spacing parameters are input through one or more of the *ALE_-
STRUCTURED_MESH_CONTROL_POINTS  cards.    The  local  coordinate  system  is 
defined using the *ALE_STRUCTURED_MESH card. 
In certain contexts it is advantageous to use structured meshes.  With structured meshes 
the  element  and  node  connectivity  are  straightforward  and  the  searching  algorithm 
used  for  ALE  coupling  is  greatly  simplified.    Also  numerous  checks  are  avoided 
because these meshes include only HEX elements. 
This new S-ALE solver supports SMP, MPP and MPP hybrid configurations.  All three 
implementations require less simulation time and memory usage than the regular ALE 
solver.    We,  therefore,  encourage  using  the  S-ALE  solver  when  the  ALE  mesh  is 
structured. 
The S-ALE solver uses the same set of keyword cards as the regular ALE solver with the 
only  exception  being  this  keyword.    Once  an  ALE  mesh  is  generated  using  *ALE_-
STRUCTURED_MESH  card  this  card  invokes  the  S-ALE  and  performs  the  ALE 
advection  timestep.    For  fluid  structured  interaction  using  the  *CONSTRAINED_-
LARGANGE_IN_SOLID card S-ALE uses a much faster searching algorithm that takes 
advantage of the mesh structure.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MSHID 
DPID 
NBID 
EBID 
Type 
Default 
I 
0 
I 
none 
  Card 2 
1 
2 
I 
0 
3 
I 
0 
4 
5 
6 
7 
8 
Variable 
CPIDX 
CPIDY 
CPIDZ 
NID0 
LCSID 
Type 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none
VARIABLE   
DESCRIPTION
MSHID 
DPID 
NBID 
EBID 
CPIDX, CPIDY, CPIDZ 
S-ALE Mesh ID.  A unique number must be specified. 
Default  Part  ID.    The  elements  generated  will  assigned
to DPID.  This part contains no material including only
the  mesh. 
is  automatically
generated  during  the  input  phase  and  contains  neither 
material  nor  element  formulation  information.    Please
see Remark 1. 
  This  part  definition 
Nodes  are  generated  and  assigned  with  node  IDs
starting from NBID.  
Elements  are  generated  and  assigned  with  element  IDs
starting from EBID.  
Control  point  IDs  defining  node  ID/value  pairs  along
each  local  axis.    See  *ALE_STRUCTURED_MESH_-
CONTROL_POINTS. 
NID0 
  During  the
NID0  sets  the  mesh’s  origin  node. 
simulation,  prescribed  motion  applied  to  this  node
applies to the entire structure S-ALE mesh. 
LCSID 
Local coordinate system ID.  Please see Remark 2. 
Remarks: 
1.  DPID.  The part specific by ID DPID wholey consists of elements and nodes.  It 
does not include material properties or integration rules.  The requirmenet that 
a  part  ID  be  specified  for  these  automatically  generated  S-ALE  solid  elements 
exusts only to satisfy the legacy rule that every element must be associated with 
a part.  Users do not need to set up the *PART card for DPID.  All PART defini-
tions used in this card only refer to mesh, not material.  
2.  LCSID.    The  local  coordinate  system  is  defined  on  the  data  cards  associated 
with  the  *DEFINE_COORDINATE  keyword.    This  local  coordinate  cordinate 
system specifies the three cardinal directions used for generating the structured 
ALE mesh.  The structured mesh can be made to rotate by specifying a rotating 
local  coordinate  system.    To  define  a  rotating  local  coordinate  system,  use  the 
*DEFINE_COORDINATE_NODES  keyword  with  FLAG = 1  and  then  apply 
prescribed motion to the three coordinate nodes. 
3.  ALES-ALE  Converter.    For  existing  ALE  models  with  rectilinear  mesh,  we 
could  use  *ALE_STRUCTURED_MESH  card  to  invoke  the  ALE  S-ALE  con-
verter.    To  invoke  this  feature,  add  a  *ALE_STRUCTURED_MESH  card  in  the 
model  input  with  CPIDX=-1/0  and  all  other  fields  blank.    It  will  then  convert 
all ALE keywords to be of S-ALE format and write the modified input in a file 
named  “saleconvrt.inc”.    The  solver  used  to  perform  the  analysis  depends  on 
the value of CPIDX.  If -1, S-ALE solver is used; if 0, ALE solver is used. 
Example: 
The following example generates a regular evenly distributed 0.2 by 0.2 by 0.2 box mesh 
having  22  nodes  along  each  direction.    The  generated  mesh  is  aligned  to  the  local 
coordinate system spefied by nodes 1, 2, 3, and 4 originating from node 1. 
All the elements inside the mesh are assigned to part 1.  Note that part 1 is not explicitly 
defined  in  the  input.    The  necessary  part  definition  is  automatically  generated  and 
contains neither material definitions nor integration rules. 
*ALE_STRUCTURED_MESH 
$    mshid      dpid      nbid      ebid 
         1         1    200001    200001 
$    cpidx     cpidy     cpidz      nid0     lcsid 
      1001      1001      1001         1       234 
*DEFINE_COORDINATE_NODES 
$      cid      nid1      nid2      nid3      flag 
       234         2         3         4         1 
*ALE_STRUCTURED_MESH_CONTROL_POINTS 
      1001 
$                 x1                  x2 
                   1                  .0 
                  22                  .2 
*NODE 
       1   0.0000000e+00   0.0000000e+00   0.0000000e+00 
       2   0.0000000e+00   0.0000000e+00   0.0000000e+00 
       3   0.1000000e+00   0.0000000e+00   0.0000000e+00 
       4   0.0000000e+00   0.1000000e+00   0.0000000e+00 
*END
*ALE_STRUCTURED_MESH_CONTROL_POINTS 
Purpose:    The  purpose  of  this  keyword  is  to  provide  spacing  information  used  by  the 
*ALE_STRUCTURED_MESH keyword to generate a 3D structured ALE mesh. 
Each  instance  of  the  *ALE_STRCUTURED_MESH_CONTROL_POINTS  card  defines  a 
one-dimensional mesh using control.  Each control point consists of a node number  and of a coordinate .  The first control point must be node 1, and 
the node number of the last point defines the total number of nodes.  Between and two 
control  points  the  mesh  is  uniform.    The  *ALE_STRUCTURED_MESH  card,  in  turn, 
defines a simple three dimensional mesh from the triple product of three *ALE_STRUC-
TURED_MESH_CONTROL_POINT one-dimensional meshes. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CPID 
Not used  Not used 
SFO 
Not used 
OFFO 
Type 
I 
Default 
None 
F 
1. 
F 
0. 
Point Cards.  Put one pair of points per card (2E20.0).  Input is terminated at the next 
keyword (“*”) card. At least two cards are required, one of which, having N = 1 is required. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
N 
X 
RATIO 
Type 
I20 
E20.0 
E20.0 
Default 
none 
none 
0.0 
  VARIABLE   
DESCRIPTION
CPID 
SFO 
Control Points ID.  A unique number must be specified.  This ID 
is  to  be  referred  in  the  three  fields  marked  up  CPIDX,  CPIDY,
CPIDZ in *ALE_STRUCTURED_MESH. 
Scale  factor  for  ordinate  value.    This  is  useful  for  simple
modifications. 
EQ.0.0: default set to 1.0.
VARIABLE   
DESCRIPTION
OFFO 
Offset for ordinate values.  See Remark 1. 
Control point node number. 
Control point position. 
Ratio  for  progressive  mesh  spacing.    Progressively  larger  or
smaller mesh will be generated between the control point that has 
nonzero  ratio  specified  and  the  control  point  following  it.    See
remark 2. 
GT.0.0: mesh size increases;  𝑑𝑙𝑛+1 =  𝑑𝑙𝑛 ∗ (1 + 𝑟𝑎𝑡𝑖𝑜) 
LT.0.0:  mesh size decreases;  𝑑𝑙𝑛+1 = 𝑑𝑙𝑛/(1 − 𝑟𝑎𝑡𝑖𝑜) 
N 
X 
RATIO 
Remarks: 
1.  Coordinates  scaling.    The  ordinate  values  are  scaled  after  the  offsets  are 
applied, i.e.: 
Ordinate  value = SFO × (Defined  value + OFFO) 
2.  Progressive  mesh  spacing.    The  formula  used  to  calculate  element  length  is 
as  follows:   𝑑𝑙𝑏𝑎𝑠𝑒 = ∣𝑥𝑒𝑛𝑑 − 𝑥𝑠𝑡𝑎𝑟𝑡∣ ∗ (𝑓𝑎𝑐𝑡𝑜𝑟 − 1)/(𝑓𝑎𝑐𝑡𝑜𝑟𝑛 − 1)    in  which   𝑑𝑙𝑏𝑎𝑠𝑒  is 
the  smallest  base  length; 𝑥𝑠𝑡𝑎𝑟𝑡  and 𝑥𝑒𝑛𝑑  are  the  coordinate  of the  start  and  end 
point 
𝑓𝑎𝑐𝑡𝑜𝑟 = 1 + 𝑟𝑎𝑡𝑖𝑜 (𝑟𝑎𝑡𝑖𝑜 > 0) 𝑜𝑟 1/(1 − 𝑟𝑎𝑡𝑖𝑜) (𝑟𝑎𝑡𝑖𝑜 < 0).  
Please note here element size either increases by 𝑟𝑎𝑡𝑖𝑜 (𝑟𝑎𝑡𝑖𝑜 > 0) or decreases by 
−𝑟𝑎𝑡𝑖𝑜/(1 − 𝑟𝑎𝑡𝑖𝑜) (𝑟𝑎𝑡𝑖𝑜 < 0) each time.  But the overall effect is the same: start-
ing from the smallest element, each time the element size is increased by |𝑟𝑎𝑡𝑖𝑜|. 
respectively; 
Example: 
1.  This example below generates a regular box mesh.  Its size is 0.2 by 0.2 by 0.2.  It is 
generated  in  a  local  coordinate  system  defined  by  three  nodes  2,  3,  4  and  originates 
from node 1. 
The  local  𝑥-axis  mesh  spacing  is  defined  by  control  points  ID  1001.    It  has  21  nodes 
evenly distributed from 0.0 to 0.2.  The local 𝑦-axis is defined by ID 1002 and has twice 
the elements of 1001.  It has 41 nodes evenly distributed from 0.0 to 0.2.  The local 𝑧-axis 
is defined by ID 1003.  It has 31 nodes and covers from 0.0 to 0.2.  The mesh is two times 
finer in the region between node 6 and node 26.
*ALE_STRUCTURED_MESH 
$    mshid      dpid      nbid      ebid 
         1         1    200001    200001 
$    cpidx     cpidy     cpidz      nid0     lcsid 
      1001      1002      1003         1       234 
*DEFINE_COORDINATE_NODES 
$      cid      nid1      nid2      nid3 
       234         2         3         4 
*ALE_STRUCTURED_MESH_CONTROL_POINTS 
      1001 
$                 x1                  x2 
                   1                  .0 
                  21                  .2 
*ALE_STRUCTURED_MESH_CONTROL_POINTS 
      1002                    
$                 x1                  x2 
                   1                  .0 
                  41                  .2 
*ALE_STRUCTURED_MESH_CONTROL_POINTS 
      1003                    
$                 x1                  x2 
                   1                  .0 
                   6                 .05 
                  26                 .15 
                  31                  .2 
*NODE 
       1   0.0000000e+00   0.0000000e+00   0.0000000e+00 
       2   0.0000000e+00   0.0000000e+00   0.0000000e+00 
       3   0.1000000e+00   0.0000000e+00   0.0000000e+00 
       4   0.0000000e+00   0.1000000e+00   0.0000000e+00 
*END 
2.    This  example  shows  how  to  generate  a  progressive  larger/smaller  mesh  spacing.  
The  mesh  geometry  is  the  same  as  the  example  above.    At  𝑥-direction  the  mesh  is 
progressively  smaller  between  node  1  and  8.    For  these  7  elements,  each  element  is 
0.1/1.1 = 9.09%  smaller than its left neighbor.  Between node 15 and node 22, the mesh 
is  progressively  larger  by  10%  each  time  in  those  7  elements.    The  7  elements  in  the 
middle between node 8 and 15 are of equal length.  
*ALE_STRUCTURED_MESH 
$    mshid      dpid      nbid      ebid 
         1         1    200001    200001 
$    cpidx     cpidy     cpidz      nid0     lcsid 
      1001      1002      1003         1       234 
*DEFINE_COORDINATE_NODES 
$      cid      nid1      nid2      nid3 
       234         2         3         4 
*ALE_STRUCTURED_MESH_CONTROL_POINTS 
      1001                    
$                 x1                  x2              ratio 
                   1                  .0               -0.1 
                   8          0.06666667 
                  15          0.13333333                0.1 
                  22                  .2
*ALE 
Purpose:    This  keyword  is  to  provide  a  convenient  utility  to  refine  existing  meshes 
generated  by  *ALE_STRUCTURED_MESH  card.    All  the  NODESET,  ELEMENTSET 
and SEGMENTSET defined using SALECPT and SALEFAC options in *SET_cards will 
be automatically updated.  This way, this card is the only modification in the input deck 
for users to define a refined S-ALE mesh. 
5 
6 
7 
8 
  Card 1 
1 
2 
Variable 
MSHID 
IFX 
Type 
I 
Default 
none 
I 
1 
3 
IFY 
I 
1 
4 
IFZ 
I 
1 
  VARIABLE   
MSHID 
IFX, IFY, IFZ 
Remarks: 
DESCRIPTION
S-ALE Mesh ID.  The ID of the Structured ALE mesh to be 
refined. 
Refinement  factor  at  each  local  direction.    Please  see
remark 1. 
1. 
IFX, IFY, IFZ prescribe how many times to refine the grid along each direction.  
They have to be integers.   
2.  This keyword provides a new modeling technique to handle the multi-material 
ALE  problems.    Compared  to  pure  Lagrange  problems,  models  contain  multi-
material ALE fluids are often time consuming and memory demanding.  So it is 
better to construct a concept model with much coarse mesh to get an estimate of 
the computational resources needed and refine the concept model mesh gradu-
ally  until  convergence  is  achieved.    This  keyword  minimized  the  user  effort 
following such procedure.   
Example: 
This  example  below  generates  two  regular  evenly  distributed  box  mesh.    Each  has  22 
nodes  along  each  direction  and  the  overall  size  is  0.2  by  0.2  by  0.2.    S-ALE  mesh  1  is
generated in a local coordinate system defined by three nodes 2,3,4 and originated from 
node 1. 
If at later times, we decided to make the mesh finer, we can simply add the following 
card.    Now  the  solid  element  set  100  would  contain  elements  ranging  between  nodes 
(1,1,23) and (45,45,45) instead of the original (1,1,11) and (22,22,22). 
*ALE_STRUCTURED_MESH_REFINE 
$    mshid       ifx       ify       ifz 
         1         2         2         2 
*ALE_STRUCTURED_MESH 
$    mshid      dpid      nbid      ebid 
         1         1    200001    200001 
$    cpidx     cpidy     cpidz      nid0     lcsid 
      1001      1001      1001         1       234 
*DEFINE_COORDINATE_NODES 
$      cid      nid1      nid2      nid3 
       234         2         3         4 
*SET_SOLID_GENERAL 
$      SID 
       100 
$      OPTION          MSHID              XMN              XMX              YMN              YMX              ZMN       
ZMX 
   SALECPT         1         1        22         1        22        11      22  
*ALE_STRUCTURED_MESH_CONTROL_POINTS 
      1001 
$                 x1                  x2 
                   1                  .0 
                  22                  .2 
*NODE 
       1   0.0000000e+00   0.0000000e+00   0.0000000e+00 
       2   0.0000000e+00   0.0000000e+00   0.0000000e+00 
       3   0.1000000e+00   0.0000000e+00   0.0000000e+00 
       4   0.0000000e+00   0.1000000e+00   0.0000000e+00 
       5   0.0000000e+00   0.0000000e+00   0.0000000e+00 
*END
*ALE 
Purpose:  This card changes a fraction of an ALE multi-material-group (AMMGID) into 
another group.  The fraction is to be specified by a *DEFINE_FUNCTION function.  The 
function take as many arguments as there are fields specified on the cards in format 2.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FR_MMG  TO_MMG 
IDFUNC 
IDSEGSET IDSLDSET NCYCSEG  NCYCSLD 
Type 
I 
I 
I 
Default 
none 
none 
None 
I 
0 
I 
0 
I 
I 
50 
50 
Variable  Cards.  Cards  defining  the  function  arguments.    Include  as  many  cards  as 
necessary.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VAR 
VAR 
VAR 
VAR 
VAR 
VAR 
VAR 
VAR 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
  VARIABLE   
FR_MMG 
TO_MMG 
DESCRIPTION
This  is  the  AMMG-SID  before  the  switch.    The  AMMG-SID 
corresponds  to  the  SID  defined  on  a  *SET_MULTI-MATERIAL_-
GROUP_LIST  (SMMGL)  card.    This  SID  refers  to  one  or  more
AMMGs.  See Remark 1. 
This  is  the  AMMG-SID  after  the  switch.    The  AMMG-SID 
corresponds  to  the  SID  defined  on  a  *SET_MULTI-MATERIAL_-
GROUP_LIST card.  This SID refers to one or more AMMGs.  See 
Remark 1. 
IDFUNC 
ID of a *DEFINE_FUNCTION function.  This function determines 
the material fraction to be switched.  See Example 1.
IDSEGSET 
IDSLDSET 
NCYCSEG 
NCYCSLD 
*ALE_SWITCH_MMG 
DESCRIPTION
ID of *SEGMENT_SET that is used to pass geometric properties to
the function specified by IDFUNC.  This field is optional. 
The  segment  center  positions  and  normal  vectors  are  computed.
For  each  ALE  element,  this  data  is  passed  to  the  function
IDFUNC  for  the  segment  the  closest  to  the  element  center.    See
Example 2. 
The  ID  of  a  *SOLID_SET  specifying  which  elements  are  affected
by this particular instance of the *ALE_SWITCH_MMG keyword.
This  field  is  optional.    If  undefined,  *ALE_SWITCH_MMG  affects
all ALE elements.  The element centers are computed and can be
used as variables in the function IDFUNC. 
Number  of  cycles  between  each  update  of  the  segment  centers
and normal vectors (if a segment set is defined).  For each update,
a  bucket  sort  is  applied  to  find  the  closest  segment  to  each  ALE
element.  If the segment nodes are fully constrained, the segment 
centers and normal vectors are computed only one time. 
Number  of  cycles  between  each  update  of  the  ALE  element
centers.    For  each  update,  a  bucket  sort  is  applied  to  find  the
closest segment to each ALE element.  If the element nodes does
not  move  (as  with  AFAC = -1  in  *CONTROL_ALE)  the  element 
centers are computed exactly once. 
VAR 
Variable rank in the following list : 
EQ.0: 
EQ.1: 
EQ.2: 
EQ.3: 
EQ.4: 
EQ.5: 
EQ.6: 
EQ.7: 
EQ.8: 
EQ.9: 
See Remark 3 
𝑥𝑥-stress for FR_MMG 
𝑦𝑦-stress for FR_MMG 
𝑧𝑧-stress for FR_MMG 
𝑥𝑦-stress for FR_MMG 
𝑦𝑧-stress for FR_MMG 
𝑧𝑥-stress for FR_MMG 
plastic strain for FR_MMG 
internal energy for FR_MMG 
bulk viscosity for FR_MMG 
EQ.10: 
volume from previous cycle for FR_MMG
GE.11 and LE.20: 
other auxiliary variables for FR_MMG
VARIABLE   
DESCRIPTION
GE.21 and LE.40:
auxiliary  variables  for  TO_MMG  (𝑥𝑥-
stress, …) 
EQ.41: 
EQ.42: 
EQ.43: 
EQ.44: 
EQ.45: 
EQ.46: 
EQ.47: 
EQ.48: 
EQ.49: 
EQ.50: 
EQ.51: 
EQ.52: 
EQ.53: 
EQ.54: 
EQ.55: 
EQ.56: 
EQ.57: 
mass for FR_MMG 
mass for TO_MMG 
volume fraction for FR_MMG 
volume fraction for TO_MMG 
material volume for FR_MMG 
material volume for TO_MMG 
time 
cycle 
𝑥-position of the ALE element center 
𝑦-position of the ALE element center 
𝑧-position of the ALE element center 
𝑥-position of the segment center 
𝑦-position of the segment center 
𝑧-position of the segment center 
𝑥-component of the segment normal 
𝑦-component of the segment normal 
𝑧-component of the segment normal 
GE.58 and LE.65: 
𝑥-positions of the ALE nodes 
GE.66 and LE.69: 
𝑥-positions of the segment nodes 
GE.70 and LE.77: 
𝑦-positions of the ALE nodes 
GE.79 and LE.81: 
𝑦-positions of the segment nodes 
GE.83 and LE.89: 
𝑧-positions of the ALE nodes 
GE.90 and LE.93: 
𝑧-positions of the segment nodes 
GE.94 and LE.101:  𝑥-velocities of the ALE nodes 
GE.102 and LE.105: 𝑥-velocities of the segment nodes 
GE.106 and LE.113: 𝑦-velocities of the ALE nodes 
GE.114 and LE.117: 𝑦-velocities of the segment nodes 
GE.118 and LE.125: 𝑧-velocities of the ALE nodes 
GE.126 and LE.129: 𝑧-velocities of the segment nodes
VARIABLE   
DESCRIPTION
GE.130 and LE.137: 𝑥-accelerations of the ALE nodes 
GE.138 and LE.141: 𝑥-accelerations of the segment nodes 
GE.142 and LE.149: 𝑦-accelerations of the ALE nodes 
GE.150 and LE.153: 𝑦-accelerations of the segment nodes 
GE.154 and LE.161: 𝑧-accelerations of the ALE nodes 
GE.162 and LE.165: 𝑧-accelerations of the segment nodes 
GE.166 and LE.173: masses of the ALE nodes 
GE.174 and LE.177: masses of the segment nodes 
EQ.178: 
EQ.179: 
EQ.180: 
rank  of  the  variable  updated  by  the 
function  
rank of the multi-material group in the set
time step 
Remarks: 
1.  Mapping.    The  multi-material  group  sets  that  are  specified  by  the  fields 
FR_MMG  and  TO_MMG  must  be  of  the  same  length.    Multi-material  groups 
are  switched  so  that,  for  instance,  the  fourth  multi-material  group  in  the  set 
FR_MMG  is  mapped  to  the  fourth  multi-material  group  in  the  set  TO_MMG.  
. 
2.  Variable  Specification.    The  variables  are  presented  to  the  function  IDFUNC 
as floating point data.  The order of the arguments appearing in the *DEFINE_-
FUNCTION should match the order of variable ranks VAR specified on Card 2 
(for this keyword).  For example, when there is one card in format 2 containing 
“47,  48,  41,  42”,  then  the  time  (47),  the  cycle  (48),  and  the  masses  (41  &  42) 
should be the first, second, third, and fourth arguments to the function defined 
on the *DEFINE_FUNCTION keyword. 
If  there  is  a  blank  column  between  2  variable  ranks,  the  list  between  these  2 
ranks is specified.  For example, if the card contains “1, ,6”, then the 6 stresses (1 
through 6) are selected as arguments .  In the case that there are 
several groups in the sets, if a variable rank VAR is repeated,  the correspond-
ing variable will be defined in the function for each group.  For instance, if the 
sets  have  3  groups  and  the  volume  fractions  of  the  2  first  groups  in  the  set 
TO_MMG are required as arguments of the function, a card in format 2 should 
have “44,44”.
3.  Variable Update  for  Several Groups.  If there is more than one group in the 
set, the function is called for each group.  For a given group with a rank in the 
set > 1 (VAR=179), some variables including the volume fraction, mass, internal 
energy may have been updated during the previous switches.  If their original 
values are required, they can be obtained by setting the first field (VAR) to 0. 
4.  Variable  Update  by  the  User.    The  variables  can  be  updated  by  the  user.    If 
VAR < 0  for  some  variables,  the  function  is  called  again  (after  the  switch)  for 
each of these variables.  VAR = 178 gives the rank of the variable for which the 
function is called.  The function’s return value is taken as the new value for this 
variable  (instead  of  the  fraction  of  material  to  switch).    If  the  rank  given  by 
VAR = 178 is zero, it means that the function is called for the switch.  Only the 
46 first variables 1 < VAR < 46, 58 < VAR < 165 and VAR = 180 can be modified. 
Example 1: 
The first example switches the material if the pressure is lower than a given value. 
*comment 
units: mks 
Switch  from  the  3rd  group  to  the  5th  one  if  the  pressure  of  the  3rd 
group  
is lower than pc : pres < pc 
Do the same for the switch from 4th to 7th  
If the switch occurs, the function frac returns 1.0.  So the whole   
material is permuted. 
xxsig 
: 
xx-stress 
of 
the 
groups 
in 
the 
1st 
*set_multi-
material_group_list 
yysig 
: 
yy-stress 
of 
the 
groups 
in 
the 
1st 
*set_multi-
material_group_list 
zzsig 
: 
zz-stress 
of 
the 
groups 
in 
the 
1st 
*set_multi-
material_group_list 
pres  : pressure 
pc    : pressure cutoff 
*ALE_SWITCH_MMG 
$#  fr_mmg    to_mmg    idfunc  idsegset  idsldset   ncycseg   ncycsld       
         1         2        10 
         1         2         3 
*set_multi-material_group_list 
1 
3,4 
*set_multi-material_group_list 
2 
5,7 
*DEFINE_FUNCTION 
10 
float frac(float xxsig, float yysig, float zzsig) 
{ 
  float pc; 
  pres = -(xxsig+yysig+zzsig)/3.0;
pc = -1000; 
  if (pres < pc) { 
    return 1.0; 
  } else { 
    return 0.0; 
  } 
 } 
Example 2: 
The second example switches the material if it goes through a segment. 
*comment 
units: mks 
Switch the 1st group to the 2nd group if the ALE element center goes  
through a segment of the set defined by idsegset = 1. 
The segment position is updated every cycle 
A fraction of the material is switched.  This fraction depends on the  
distance between the segment and element centers  
time    : 47th variable 
cycle   : 48th variable 
xsld    : 49th variable (x-position of the element center) 
ysld    : 50th variable (y-position of the element center) 
zsld    : 51th variable (z-position of the element center) 
xseg    : 52th variable (x-position of the segment center) 
yseg    : 53th variable (y-position of the segment center) 
zseg    : 54th variable (z-position of the segment center) 
xn      : 55th variable (x-component of the segment normal) 
yn      : 56th variable (y-component of the segment normal) 
zn      : 57th variable (z-component of the segment normal) 
volmat1 : 43th variable (material volume of the 1st group)   
volfrac1: 45th variable (volume fraction of the 1st group) 
segsurf : segment surface (given by 0.5*sqrt(xn*xn+yn*yn+zn*zn)) 
sldvol  : ALE element volume (given by volmat1/volfrac1) 
segcharaclen: characteristic length for the segment 
sldcharaclen: characteristic length for the solid 
xseg2sld: x-component of the vector segment center to element center 
yseg2sld: y-component of the vector segment center to element center 
zseg2sld: z-component of the vector segment center to element center 
distnormseg2sld: Distance segment-element projected on the normal 
disttangseg2sld: Distance segment-element projected on the segment plane   
*ALE_SWITCH_MMG 
$#  fr_mmg    to_mmg    idfunc  idsegset  idsldset   ncycseg   ncycsld       
         1         2        11         1                   1 
        47                  57        43        45 
*set_multi-material_group_list 
1 
1 
*set_multi-material_group_list 
2 
2 
*DEFINE_FUNCTION 
11 
float switchmmg(float time, float cycle, 
                float xsld, float ysld, float zsld,
float xseg, float yseg, float zseg, 
                float xn, float yn,  float zn, 
                float volmat1, float volfrac1) 
{ 
  float segsurf, sldvol, segcharaclen, sldcharaclen; 
  float xseg2sld, yseg2sld, zseg2sld, distnormseg2sld; 
  float xtangseg2sld, ytangseg2sld, ztangseg2sld, disttangseg2sld; 
  float frac; 
  segsurf = sqrt(xn*xn+yn*yn+zn*zn); 
  if (segsurf != 0.0) { 
    xn = xn/segsurf; 
    yn = yn/segsurf; 
    zn = zn/segsurf; 
  } 
  segsurf = 0.5*segsurf; 
  sldvol = volmat1/volfrac1; 
  segcharaclen = 0.5*sqrt(segsurf); 
  sldcharaclen = 0.5*sldvol**(1.0/3.0); 
  xseg2sld = xsld-xseg; 
  yseg2sld = ysld-yseg; 
  zseg2sld = zsld-zseg; 
  distnormseg2sld = xseg2sld*xn+yseg2sld*yn+zseg2sld*zn; 
  xtangseg2sld = xseg2sld-distnormseg2sld*xn; 
  ytangseg2sld = yseg2sld-distnormseg2sld*yn; 
  ztangseg2sld = zseg2sld-distnormseg2sld*zn; 
  disttangseg2sld = xtangseg2sld*xtangseg2sld+ 
                  ytangseg2sld*ytangseg2sld+ 
                  ztangseg2sld*ztangseg2sld; 
  disttangseg2sld = sqrt(disttangseg2sld); 
  if (disttangseg2sld <= segcharaclen &&  
      distnormseg2sld <= sldcharaclen) { 
    sldcharaclen = 2.0*sldcharaclen; 
    frac = distnormseg2sld/sldcharaclen; 
    frac = 0.5-frac; 
    return frac; 
  } else { 
    return 0.0; 
  } 
}
*ALE_TANK_TEST 
Purpose:  Control volume airbags (*AIRBAG_) only require two engineering curves to 
define  gas  inflator,  i.e.  𝑚̇ (𝑡)  and  𝑇̅̅̅̅̅
gas(𝑡);  those  two  curves  can  be  experimentally 
measured.  However, the ALE inflator needs one additional state variable - the inlet gas 
velocity which is impractical to obtain.  This keyword is to provide such curve through 
an engineering approximation. 
It  takes  two  curves  from  the  accompanying  *SECTION_POINT_SOURCE  as  input.    It 
assumes  inflator  gas  under  choking  condition  to  generate  velocity  curve.    During  this 
process, the original curves, 𝑚̇ (𝑡) and 𝑇̅̅̅̅̅
gas(𝑡), are modified accordingly. 
It  complements  and  must  be  used  together  with  the*SECTION_POINT_SOURCE 
command.  Please see *SECTION_POINT_SOURCE for additional information. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MDOTLC 
TANKV 
PAMB 
PFINAL  MACHL 
VELMAX 
AORIF 
Type 
Default 
I 
0 
I 
I 
I 
F 
F 
F 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
AMGIDG 
AMGIDA  NUMPNT 
Type 
Default 
I 
0 
I 
0 
I 
50 
  VARIABLE   
MDOTLC 
TANKV 
DESCRIPTION
LCID  for  mass  flow  rate  as  a  function  of  time.    This  may  be
obtained directly from the control-volume type input data. 
Volume  of  the  tank  used  in  a  tank  test  from  which  the  tank
pressure  is  measured,  and  𝑚̇ (𝑡)  and  𝑇̅̅̅̅gas(𝑡)  are  computed  from 
this tank pressure data.
VARIABLE   
DESCRIPTION
PAMB 
The pressure inside the tank before jetting (usually 1bar). 
PFINAL 
The final equilibrated pressure inside the tank from the tank test.  
MACHL 
VELMAX 
AORIF 
A  limiting  MACH  number  for  the  gas  at  the  throat  (MACH = 1 
preferred).   
Maximum  allowable  gas  velocity  across  the  inflator  orifice  (not
preferred). 
Total  inflator  orifice  area  (optional,  only  needed  if  the  *SEC-
TION_POINT_SOURCE card is not used). 
AMGIDG 
The ALE multi-material group ID (AMMGID) of the gas. 
AMGIDA 
The ALE multi-material group ID (AMMGID) of the air. 
NUMPNT 
The  number  of  points 
NUMPNT = 0, defaults to 50 points. 
in  𝑚̇ (𝑡)  and  𝑇̅̅̅̅gas(𝑡)  curves. 
  If 
Remarks: 
In an airbag inflator tank test, the tank pressure data is measured.  This pressure is used 
to  derive  𝑚̇ (𝑡)  and  to  estimate  𝑇̅̅̅̅gas(𝑡),  the  stagnation  temperature  of  the  inflator  gas.  
This  is  done  by  applying  a  lumped-parameter  method  to  the  system  of  conservation 
equations using an equation of state. 
Together  𝑚̇ (𝑡)  and  𝑇̅̅̅̅gas(𝑡)  provide  enough  information  to  model  an  airbag  with  the 
control volume method .  However, for an ALE or Eulerian fluid-
structure interaction analysis, the gas velocity, 𝑣(𝑡), and density, 𝜌(𝑡), at the inlet must 
be  computed.    But,  since  only  𝑚̇ (𝑡)  is  known,  additional  assumptions  must  be  made 
about the inlet conditions.  If 𝑣(𝑡) and 𝜌(𝑡) are calculated outside of LS-DYNA, then LS-
DYNA  combines  them  with  𝑚̇ (𝑡)  and  𝑇̅̅̅̅gas(𝑡)  to  obtain  𝑇̅̅̅̅gas corrected(𝑡),  𝑣(𝑡)  and  𝜌(𝑡) 
which are sufficient input for an ALE calculation. 
The  curves  𝑣(𝑡)  and  𝜌(𝑡)  need  not  be  calculated  outside  of  LS-DYNA  as  LS-DYNA 
features  a  method  for calculating  them  itself.    This  card,  *ALE_TANK_TEST,  activates 
this  capability.    Thus,  with  the  combination  of  this  card  and  the  *SECTION_POINT_-
SOURCE card, LS-DYNA can proceed directly from the control volume method input, 
𝑚̇ (𝑡)  and  𝑇̅̅̅̅gas(𝑡),  to  an  ALE  or  Eulerian  fluid-structure  interaction  analysis.    The  user 
does not have to do the conversion himself.
If the *ALE_TANK_TEST card is present: 
1.  The definitions of the relative volume, 𝑉(𝑡), and the velocity, 𝑣(𝑡), curves in the 
*SECTION_POINT_SOURCE  card  will  be  ignored  in  favor  of  those  computed 
by LS-DYNA. 
2.  The 𝑚̇ (𝑡)curve is read in on *ALE_TANK_TEST card. 
3.  The 𝑇gas(𝑡) curve (stagnation temperature), as opposed to  𝑇gas corrected(𝑡), is read 
in on *SECTION_POINT_SOURCE card. 
There  is  a  subtle,  but  important,  distinction  between  the  two  temperatures.  
𝑇gas(𝑡)  is  derived  directly  from  the  tank  pressure  data  based  on  a  lump-
parameter approach, whereas 𝑇gas corrected(𝑡) is computed from 𝑚̇ (𝑡) and 𝑇gas(𝑡) 
with additional isentropic and sonic flow assumptions for the maximum veloci-
ty  at  an  orifice.    𝑇gas corrected(𝑡)  is  most  appropriately  interpreted  as  the  static 
temperature.  These assumptions provide a necessary and physically reasonable 
supplement to the governing equation, 
𝑚̇ (𝑡) = 𝜌(𝑡)𝑣(𝑡)𝐴 
in  which  only𝑚̇ (𝑡)  and  𝐴  are  known  leaving  two parameters: 𝜌(𝑡),  and 𝑣(𝑡)  as 
unkown. 
4.  The inflator area is computed from the *SECTION_POINT_SOURCE card that 
has  the  AMMGID  of  the  inflator  gas  in  the  *ALE_TANK_TEST  card.    If  the 
*BOUNDARY_AMBIENT_EOS card is used instead of the *SECTION_POINT_-
SOURCE card, then the area may be input in this *ALE_TANK_TEST card.   
5.  The  reference  density  of  the  propellant  “gas”,  𝜌0,  is  computed  internally  and 
automatically  used  for  the  calculation.    The  𝜌0  value  from  the  *MAT_NULL 
card is ignored.   
Example: 
Consider a tank test model consists of the inflator gas (PID 1) and the air inside the tank 
(PID 2).  The following information from the control volume model is available: 
•  𝑚̇ (𝑡) (LCID 1 is from control volume model input). 
•  𝑇̅̅̅̅gas(𝑡) (LCID 2 is from control volume model input). 
•  Volume of the tank used in the inflator tank test. 
•  Final equilibrated pressure inside the tank. 
•  Ambient pressure in the air. 
Also available are:
•  The nodal IDs of the nodes defining the orifice holes through which the gas flows 
into the tank. 
•  The area associated with each hole (the node is assumed to be at the center of this 
area). 
•  The vector associated with each hole defining the direction of flow. 
In the input below LCID 1 and 2 are 𝑚̇ (𝑡) and 𝑇̅̅̅̅gas(𝑡), respectively.  LCID 4 and 5 will be 
ignored when the *ALE_TANK_TEST card is present.  If it is not present, all 3 curves in 
the  *SECTION_POINT_SOURCE  card  will  be  used.    When  the  *SECTION_POINT_-
SOURCE card is present, the element formulation is equivalent to an ELFORM = 11. 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 
*PART 
inflator gas 
$      PID     SECID       MID     EOSID      HGID      GRAV    ADPOPT      TMID 
         1         1         1         0         0         0         0         0 
*PART 
air inside the tank 
$      PID     SECID       MID     EOSID      HGID      GRAV    ADPOPT      TMID 
         2         2         2         0         0         0         0         0 
*SECTION_SOLID 
$    SECID    ELFORM       AET 
         2        11         0 
*ALE_MULTI-MATERIAL_GROUP 
$      SID   SIDTYPE 
         1         1        
         2         1        
*SECTION_POINT_SOURCE 
$    SECID     LCIDT  LCIDVOLR   LCIDVEL      <= 3 curves in tempvolrvel.k file 
         1         2         4         5 
$   NODEID    VECTID      AREA   
     24485         3    15.066          
       ...      
     24557         3    15.066 
*ALE_TANK_TEST 
$   MDOTLC     TANKV      PAMB    PFINAL     MACHL    VELMAX     AORIF 
         1     6.0E7    1.0E-4  5.288E-4       1.0       0.0 
$   AMGIDG    AMGIDA    NUMPNT 
         1         2        80 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8
*ALE_UP_SWITCH 
Purpose:  For the simulation of airbag inflation process, this card allows the switching 
from an ALE computation to a control volume (CV) or uniform pressure (UP) method 
at a user-defined switch time. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
UPID 
SWTIME 
F 
1.0e+16 
Type 
Default 
Remark 
I 
0 
1 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FSI_ID1 
FSI_ID2 
FSI_ID3 
FSI_ID4 
FSI_ID5 
FSI_ID6 
FSI_ID7 
FSI_ID8 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
Additional card for UPID = 0 (or not defined). 
Optional 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
SIDTYPE  MMGAIR  MMGGAS
Type 
Default 
I 
0 
I 
0 
I 
0 
I
VARIABLE   
UPID 
DESCRIPTION
An  ID  defines  a  corresponding  *AIRBAG_HYBRID_ID  card  for 
use in an ALE-method-switching-to-CV-method simulation.  The 
simulation starts with ALE computational method, then switches
to a CV (or UP) method at some given time. 
EQ.0: (or  blank)  The  code  will  construct  an  equivalent 
*AIRBAG_HYBRID_ID  card  automatically  internally, 
(default).  The 3rd optional line is then a required input. 
NE.0: An ID points to a corresponding *AIRBAG_HYBRID_ID 
card  which  must  be  defined  for  use  after  the  switch.    If
UPID is defined, do not define the 3rd optional card. 
SWTIME 
The  time  at  which  the  computation  does  a  switch  from  an  ALE-
method-to-CV-method.   
FSI_ID1, …, 
FSI_ID8 
Coupling  IDs  for  one  or  more  ALE  fluid-structure-interaction 
(FSI) 
cards. 
*CONSTRAINED_LAGRANGE_IN_SOLID_ID 
These  couplings  are  deleted  during  the  2nd,  CV  computational 
phase. 
SID 
A set ID defines the Lagrangian parts which make up the airbag. 
SIDTYPE 
Set  ID  type  for  the  above  SETID  (following  the  conventions  in
*AIRBAG_HYBRID card). 
EQ.0: SID is a segment set ID (SGSID). 
NE.0: SID is a part set ID (PSID). 
MMGAIR 
The AMMG (ALE multi-material group) ID of surrounding air. 
MMGGAS 
The AMMG ID of inflator gas injected into the airbag. 
Remarks: 
1. 
If  UPID  is  zero  or  blank,  optional  card  3  must  be  defined.    LSDYNA  will 
construct an equivalent *AIRBAG_HYBRID_ID card automatically.
*ALE_UP_SWITCH 
Consider  an  airbag  model  with  a  2-phase  simulation:    an  ALE  calculation  being 
switched  to  a  CV  method.    During  the  CV  phase,  the  simulation  is  defined  by  an 
*AIRBAG_HYBRID_ID card. 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
*ALE_UP_SWITCH 
$    UP_ID   SW_time 
    100000    2.0000 
$ FSI_ID_1  FSI_ID_2  FSI_ID_3  FSI_ID_4  FSI_ID_5  FSI_ID_6  FSI_ID_7  FSI_ID_8 
         1         2 
$-------------------------------------------------------------------------------
*AIRBAG_HYBRID_ID 
$       ID 
    100000 
$      SID    SIDTYP      RBID      VSCA      PSCA      VINI       MWD      SPSF 
         2         1         0       1.0       1.0       0.0       0.0       0.0 
$ 2   ATMT      ATMP      ATMD        GC        CC 
      293.  1.0130e-4  1.200E-9    8.3143        1. 
$      C23     LCC23       A23     LCA23      CP23     LCP23      AP23    LCAP23 
$      OPT     PVENT      NGAS 
                             4 
$bac LCIDM     LCIDT   NOTUSED        MW     INITM         A         B         C 
      1001      1002           0.0288691       1.0     28.98 
$    FMASS 
$air LCIDM     LCIDT   NOTUSED        MW     INITM         A         B         C 
      1600      1603            28.97E-3       0.0     26.38  8.178e-3 -1.612e-6 
$    FMASS 
$pyroLCIDM     LCIDT   NOTUSED        MW     INITM         A         B         C 
      1601      1603            43.45E-3       0.0     32.87  2.127e-2 -5.193E-6 
$    FMASS 
$sto_LCIDM     LCIDT   NOTUSED        MW     INITM         A         B         C 
      1602      1603            39.49E-3       0.0     22.41  2.865e-3 -6.995e-7 
$    FMASS 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
Example 2: 
Consider  the  same  airbag  model  with  the  same  2-phase  simulation.    However,  all  the 
*AIRBAG_HYBRID_ID  card  definitions  are  extracted  automatically  from  the  ALE 
model.    There  is  no  need  to  define  the  *AIRBAG_HYBRID_ID  card.    The  3rd  optional 
card is required. 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
*ALE_UP_SWITCH 
$    UP_ID   SW_time 
$   100000    2.0000 
         0    2.0000 
$ FSI_ID_1  FSI_ID_2  FSI_ID_3  FSI_ID_4  FSI_ID_5  FSI_ID_6  FSI_ID_7  FSI_ID_8 
         1         2 
$    SETID    SETYPE   MMG_AIR   MMG_GAS 
         2         1         2         1 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8
The keyword *BOUNDARY provides a way of defining imposed motions on boundary 
nodes.  The keyword control cards in this section are defined in alphabetical order: 
*BOUNDARY_ACOUSTIC_COUPLING 
*BOUNDARY_ACOUSTIC_IMPEDANCE 
*BOUNDARY_ACOUSTIC_MAPPING 
*BOUNDARY_ALE_MAPPING 
*BOUNDARY_AMBIENT 
*BOUNDARY_AMBIENT_EOS 
*BOUNDARY_CONVECTION_OPTION 
*BOUNDARY_COUPLED 
*BOUNDARY_CYCLIC 
*BOUNDARY_DE_NON_REFELECTING 
*BOUNDARY_ELEMENT_METHOD_OPTION 
*BOUNDARY_FLUX_OPTION 
*BOUNDARY_MCOL 
*BOUNDARY_NON_REFLECTING 
*BOUNDARY_NON_REFLECTING_2D 
*BOUNDARY_PAP 
*BOUNDARY_PORE_FLUID_OPTION 
*BOUNDARY_PRECRACK 
*BOUNDARY_PRESCRIBED_ACCELEROMETER_RIGID 
*BOUNDARY_PRESCRIBED_FINAL_GEOMETRY 
*BOUNDARY_PRESCRIBED_MOTION_{OPTION1}_{OPTION2} 
*BOUNDARY_PRESCRIBED_ORIENTATION_RIGID_OPTION
*BOUNDARY_PWP_OPTION 
*BOUNDARY_RADIATION_OPTION 
*BOUNDARY_SLIDING_PLANE 
*BOUNDARY_SPC_{OPTION1}_{OPTION2}_{OPTION3} 
*BOUNDARY_SPC_SYMMETRY_PLANE_OPTION 
*BOUNDARY_SPH_FLOW 
*BOUNDARY_SPH_NON_REFLECTING 
*BOUNDARY_SPH_SYMMETRY_PLANE 
*BOUNDARY_SYMMETRY_FAILURE 
*BOUNDARY_TEMPERATURE_OPTION 
*BOUNDARY_THERMAL_BULKFLOW_{OPTION1}_{OPTION2} 
*BOUNDARY_THERMAL_BULKNODE 
*BOUNDARY_THERMAL_WELD 
*BOUNDARY_THERMAL_WELD_TRAJECTORY 
*BOUNDARY_USA_SURFACE
*BOUNDARY_ACOUSTIC_COUPLING_{OPTION} 
There are two forms of this keyword command: 
1. 
for coupling of surfaces with coincident nodes 
*BOUNDARY_ACOUSTIC_COUPLING 
2. 
for coupling surfaces without coincident nodes 
*BOUNDARY_ACOUSTIC_COUPLING_MISMATCH 
Purpose:    Define  a  segment  set  for  acoustic  coupling  of  structural  element  faces  and 
acoustic volume elements (type 8 and type 14 solid elements.)   
If the mismatch option is not used, then this command couples either one side of a shell 
or  solid  element  structure  or  both  sides  of  a  shell  structure  to  acoustic  elements.    The 
segments in the segment set should define the structural surface for which coupling is 
intended.    The  nodal  points  of  the  structural  segments  must  be  coincident  with  the 
nodal  points  for  the  fluid  element  faces  on  either  side  of  the  structural  segments.    If 
fluid exists on just one side of the structural segments, and the nodes are merged, then 
the input data in this section is not required.  The coupling will happen automatically.  
However,  if  fluid  is  on  both  sides  of  the  structural  segments,  then  this  input  data  is 
required  and  the  nodes  should  not  be  merged;  two-sided  coupling  will  not  properly 
apply loads when the interface nodes are merged out. 
If  the  mismatch  option  is  used,  then  this  command  permits  the  coupling  of  acoustic 
fluid  volume  elements  with  one  side  of  a  structural  element  when  the  meshes  of  the 
fluid and structural models are moderately mismatched.  In this case, it is possible that 
most fluid and structural nodes will not be coincident.  None of the fluid and structural 
nodes  at  the  interface  should  be  merged  together.    The  segments  in  the  segment  set 
should define the structural surface and, following a right hand rule, the normal vector 
for  the  segments  should  point  at  the  fluid  volume  elements  with  which  coupling  is 
intended.  If coupling is required on both sides of a structural shell element, duplicate 
segments  with  opposite  normal  vectors  should  be  defined.    Every  segment  in  the 
segment set must couple with the fluid volume at some integration point, but it is not 
necessary that all integration points on the segment couple with the fluid.  The meshes 
do  not  have  to  be  mismatched  to  use  mismatched  coupling,  as  long  as  the  fluid  and 
structural nodes are not merged.
Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
Type 
I 
Default 
none 
  VARIABLE   
DESCRIPTION
SSID 
Segment set ID, see *SET_SEGMENT 
Remarks: 
1.  For the stability of the acoustic-structure coupling, the following condition must 
be satisfied: 
2𝜌𝑎𝐷
𝜌𝑠𝑡𝑠
< 5 
where 𝜌𝑎  is  the  density  of  the  acoustic  medium, 𝐷  is  the  total  thickness  of  the 
acoustic elements adjacent to the structural element, 𝜌𝑠 is the density, and 𝑡𝑠 is 
the thickness of the structural shell element.  If the structural element is a solid 
or  thick  shell  element,  then  ts  should  be  half  the  thickness  of  the  element.    If 
coupling is on both sides of the structural elements, then ts should also be half 
the thickness of the structural element. 
2. 
In  mismatched  coupling,  free  fluid  faces  are  considered  for  coupling  with  the 
structural  segments  if  they  are  near  one  another  and  if  they  face  each  other.  
Faces  and  segments  that  differ  in  orientation  by  more  than  45  degrees  are  ex-
cluded.    In  regions  of  high  curvature  the  surfaces  therefore  need  to  be  more 
similar than  when the surfaces are flat.   If a fluid face couples with any struc-
tural  segment,  then  all  four  integration  points  on  the  fluid  face  must  couple 
with some structural segment.  Fluid faces may not be partially coupled.  Struc-
tural segments are allowed to be partially coupled. 
3.  The  mismatched  coupling  process  dumps  two  LS-DYNA  files  that  can  be 
imported into LS-PrePost for review of the results of the coupling process.  File 
“bac_str_coupling.dyn” contains shell elements where structural segments have 
coupled with the fluid and mass elements at structural integration points with 
coupling.    When  the  messag  file  indicates  that  some  structural  segments  have 
partial coupling, this file can be used to check the unconnected segment integra-
tion  points.    File  “bac_flu_coupling.dyn”  contains  shell  elements  where  free
fluid faces have coupled with the structural segments and mass elements at free 
fluid  face  integration  points  with  coupling.    These  files  are  only  for  visualiza-
tion of the coupling and serve no other purpose.
*BOUNDARY_ACOUSTIC_IMPEDANCE 
Purpose:  Define a segment set to prescribe the acoustic impedance of acoustic volume 
element (type 8 and type 14 solid elements) faces.   
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
ZEE 
Type 
I 
F 
Default 
none 
none 
  VARIABLE   
DESCRIPTION
Segment set ID, see *SET_SEGMENT 
Value of the acoustic impedance ρc 
SSID 
ZEE 
Remarks: 
1.  The  effect  of  the  boundary  impedance  on  the  acoustic  cavity  response  is 
incorporated in the forcing vector.  Solutions are conditionally stable, with low 
values  of  impedance  relative  to  the  impedance  of  the  *MAT_ACOUSTIC  ele-
ments  causing  instabilities.    Reducing  the  factor  of  safety  on  the  time  step  ex-
tends  the  range  of  applicability,  however  it  is  recommended  that  pressure 
release  conditions  be  handled  by  leaving  the  boundary  free  rather  than  by 
providing  a  relatively  low  boundary  acoustic  impedance  value.    A  warning  is 
issued  if the boundary impedance value is less than 25 percent of the *MAT_-
ACOUSTIC impedance.  A value less than 1 percent of the *MAT_ACOUSTIC 
impedance is considered to be an error. 
 Special  allowance  is  made  for  cases  when  both  *LOAD_SEGMENT  set 
pressures and the *BOUNDARY_ACOUSTIC_IMPEDANCE are defined on the 
same  segments.    In  this  event  a  nonreflecting  entrant  boundary  condition  is 
assumed.  The pressures in the LOAD_SEGMENT_SET definition are treated as 
incoming  incident  pressure.    Pressure  waves  within  the  *MAT_ACOUSTIC 
domain striking this boundary will exit the model.  In contrast, a *LOAD_SEG-
MENT_SET  on  *MAT_ACOUSTIC  volume  faces  in  the  absence  of  *BOUND-
ARY_ACOUSTIC_IMPEDANCE  acts  as  a  time-dependent,  total  pressure 
constraint  and  pressure  waves  within  the  *MAT_ACOUSTIC  domain  striking 
this boundary will be reflected back into the model.
2.
*BOUNDARY_ACOUSTIC_MAPPING 
Purpose:    Define  a  set  of  elements  or  segments  on  structure  for  mapping  structural 
nodal velocity to acoustic volume boundary.    
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
STYP 
Type 
I 
Default 
none 
I 
0 
  VARIABLE   
DESCRIPTION
SSID 
STYP 
Set or part ID 
Set type: 
EQ.0: part set ID, see *SET_PART, 
EQ.1: part ID, see *PART, 
EQ.2: segment set ID, see *SET_SEGMENT. 
Remarks: 
1. 
If acoustic elements are not overlapping with structural elements, this keyword 
passes  structural  velocity  to  acoustic  volume  boundary,  for  subsequent  fre-
quency domain acoustic computation.
*BOUNDARY_ALE_MAPPING 
Purpose:    This  card  maps  ALE  data  histories  from  a  previous  run  to  a  region  of 
elements.  Data are read or written in a mapping file called by the prompt “map=” on 
the  command  line  .    To  map  data  at  the  initial  time  (not  the 
histories)  to  all  the  ALE  domain  (not  just  a  region  of  elements)  see  *INITIAL_ALE_-
MAPPING. 
The following transitions are allowed: 
1D → 2D 
1D → 3D 
2D → 2D 
2D → 3D 
3D → 3D 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
TYP 
AMMSID 
IVOLTYP 
BIRTH 
DEATH 
DTOUT 
Type 
I 
I 
I 
I 
F 
F 
F 
Default 
none 
none 
none 
none 
0.0 
1020 
  Card 2 
1 
2 
Variable 
THICK 
RADIUS 
Type 
F 
F 
3 
X1 
F 
4 
Y1 
F 
5 
Z1 
F 
6 
X2 
F 
time 
step 
7 
Y2 
F 
8 
INI 
I 
0 
8 
Z2 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 3 
Variable 
1 
XO 
Type 
F 
2 
YO 
F 
3 
ZO 
F 
4 
5 
6 
7 
8 
VECID 
I 
Default 
0.0 
0.0 
0.0 
none
VARIABLE   
DESCRIPTION
ID 
TYP 
Part ID or part set ID or element set ID 
Type of “ID” : 
EQ.0: part set ID. 
EQ.1: part ID. 
EQ.2: shell set ID. 
EQ.3: solid set ID. 
AMMSID 
IVOLTYP 
Set  ID  of  ALE  multi-material  groups  defined  in  *SET_MULTI-
MATERIAL_GROUP.  See Remark 1. 
Type of volume containing the selected elements for the mapping.
The  absolute  value  of  IVOLTYPE  indicates  the  type  of  volume
and the sign indicates whether the data is being read of written. 
Volume Type 
|IVOLTYP|.EQ.1: Spherical surface with thickness (THICK). 
|IVOLTYP|.EQ.2: Box. 
|IVOLTYP|.EQ.3: Cylindrical surface with thickness (THICK) 
|IVOLTYP|.EQ.4: All the elements defined by ID. 
Read/Write 
IVOLTYP.LT.0:  data  from  the  mapping  file  are  read  for  the
elements of this volume. 
IVOLTYP.GT.0:  data  from  the  elements  of  this  volume  are
written in the mapping file. 
BIRTH 
DEATH 
Birth time to write or read the mapping file.  If a mapping file is
written, the next run reading this file will begin at time BIRTH if
this parameter for this next run is not larger. 
Death time to write or read the mapping file.  If a mapping file is
written, the next run will stop to read this file at time DEATH if
this parameter for this next run is not smaller. 
DTOUT 
Time  interval  between  outputs  in  the  mapping  file.    This
parameter is only used to write in the mapping file.
VARIABLE   
DESCRIPTION
INI 
Flag to initialize all the ALE domain of the next run: 
EQ.0: No initialization 
EQ.1:  Initialization.  *INITIAL_ALE_MAPPING will have to be 
in  the  input  deck  of  the  next  run  to  read  the  data  from
the mapping file.  The initial time of the next run will be
BIRTH. 
THICK 
Thickness for the element selection using surfaces. 
RADIUS 
Radius for abs(IVOLTYP) = 1 and abs(IVOLTYP) = 3. 
If abs(IVOLTYP).EQ.1: 
X1 
Y1 
Z1 
X1 is the 𝑥-coordinate of the sphere center. 
Y1 is the 𝑦-coordinate of the sphere center. 
Z1 is the 𝑧-coordinate of the sphere center. 
X2, Y2, Z2 
Ignored 
If abs(IVOLTYP).EQ.2: 
X1 
Y1 
Z1 
X2 
Y2 
Z2 
X1 is the 𝑥-coordinate of the box’s minimum point. 
Y1 is the 𝑦-coordinate of the box’s minimum point. 
Z1 is the 𝑧-coordinate of the box’s minimum point. 
X2 is the 𝑥-coordinate of the box’s maximum point. 
Y2 is the 𝑦-coordinate of the box’s maximum point. 
Z2 is the 𝑧-coordinate of the box’s maximum point.
VARIABLE   
DESCRIPTION
If abs(IVOLTYP).EQ.3: 
X1 
Y1 
Z1 
X2 
Y2 
Z2 
X1 is the 𝑥-coordinate of a point on the cylinder’s axis. 
Y1 is the 𝑦-coordinate of a point on the cylinder’s axis. 
Z1 is the 𝑧-coordinate of a point on the cylinder’s axis. 
X2 is the 𝑥-coordinate of a vector parallel to the cylinder’s axis. 
Y2 is the 𝑦-coordinate of a vector parallel to the cylinder’s axis. 
Z2 is the 𝑧-coordinate of a vector parallel to the cylinder’s axis. 
If abs(IVOLTYP).EQ.4: 
X1, Y1, Z1 
ignored 
X2, Y2, Z2 
ignored 
End if 
X0 
Y0 
Z0 
Origin position in global 𝑥-direction.  See Remark 2. 
Origin position in global 𝑦-direction.  See Remark 2. 
Origin position in global 𝑧-direction.  See Remark 2. 
VECID 
ID  of  the  symmetric  axis  defined  by  *DEFINE_VECTOR.    See 
Remark 3. 
Remarks: 
1.  Mapping  of  Multi-Material  Groups.    The  routines  of  this  card  need  to  know 
which  mesh  will  be  initialized  with  the  mapping  data  and  more  specifically 
which multi-material groups.  The first 2 parameters (ID and TYP) defines the 
mesh  and  the  third  one  (AMMSID)  refer  to  the  *SET_MULTI-MATERIAL_-
GROUP_LIST card.  This card will define a list of material groups in the current 
run.    The  rank  in  this  list  should  match  the  rank  of  the  multi-material  groups 
from  the  previous  run  (as  a  reminder  the  ranks  of  multi-material  groups  are 
defined  by  *ALE_MULTI-MATERIAL_GROUP).    For  instance,  if  the  previous 
model has 3 groups, the current one has 5 groups, and the following mapping is 
wanted:
The 1st group (previous) ⇒  the 3rd group (current), 
The 2nd group (previous) ⇒  the 5th group (current) and, 
The 3rd group (previous) ⇒  the 4th group (current). 
Then, the *SET_MULTI-MATERIAL_GROUP_LIST card should be as follows: 
*SET_MULTI-MATERIAL_GROUP_LIST 
300 
3,5,4 
2.  Origin.  The data can be mapped in different parts of the mesh by defining the 
origin of the coordinate system (X0, Y0, Z0). 
3.  Orientation  Vector:  VECID.    For  a  mapping  file  created  by  a  previous 
asymmetric model, the symmetric axis orientation in the current model is speci-
fied by VECID.  For a mapping file created by a 3D or 1D spherical model, the 
vector  VECID  is  read  but  ignored.    The  definitions  of  X0,  Y0,  Z0  and  VECID 
change in the case of the following mappings: 
a)  plain strain 2D (ELFORM = 13 in *SECTION_ALE2D) to plain strain 2D 
b)  plain strain 2D to 3D 
While, VECID still defines the y-axis in the 2D domain, the 3 first parameters in 
*DEFINE_VECTOR,  additionally,  define  the  location  of  the  origin.    The  3  last 
parameters  defines  a  position  along  the  y-axis.    For  this  case  when  2D  data  is 
used in a 3D calculation the point X0, Y0, Z0 together with the vector, VECID, 
define the plane. 
4.  Mapping  File.    To  make  one  mapping:  only  the  command-line  argument 
“map=” is necessary.  If IVOLTYP is positive, the mapping file will be created 
and ALE data histories will be written in this file.  If IVOLTYP is negative the 
mapping file will be read and ALE data histories will be used to interpolate the 
ALE  variables  of  the  selected  elements.    This  file  contains  the  following  nodal 
and element data: 
•  nodal coordinates  
•  nodal velocities 
•  part ids 
•  element connectivities 
•  element centers 
•  densities 
•  volume fractions
•  stresses 
•  plastic strains 
•  internal energies 
•  bulk viscosities 
•  relative volumes 
5.  Successive  Mappings.    To  make  several  successive  mapping:  the  prompt 
“map1=”  is  necessary.    If  IVOLTYP is  positive  and  the  prompt  “map1=”  is  in 
the  command  line,  the  ALE  data  are  written  to  the  mapping  file  given  by 
“map1=”.  If IVOLTYP is negative and the prompt “map=” is in the command 
line, ALE data are read from the mapping file given by “map=”.
*BOUNDARY_AMBIENT 
Purpose:    This  command  defines  ALE  “ambient”  type  element  formulations 
(please see Remarks 1, 2 and 5). 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SETID 
MMG 
AMBTYP 
Type 
I 
I 
I 
Default 
none 
none 
none 
Optional Card.  Additional optional card for AMBTYP = 4 with curves 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID1 
LCID2 
Type 
I 
I 
Default 
none 
none 
  VARIABLE   
SETID 
DESCRIPTION
The ambient element set ID for which the thermodynamic state is
being defined.  The element set can be *SET_SOLID for a 3D ALE 
model, *SET_SHELL for a 2D ALE model or *SET_BEAM for a 1D 
ALE model.  
MMG 
ALE multi-material group ID. 
AMBTYP 
Ambient element type: 
EQ.4: Pressure inflow/outflow  
EQ.5: Receptor 
for  blast 
load
DESCRIPTION
A  load  curve  ID  for  internal  energy  per  unit  reference  volume
(Please see Remark 4 and  read the beginning of the EOS section 
for  details).    If  *EOS_IDEAL_GAS  is  being  used,  this  ID  then 
refers to a temperature load curve ID. 
Load  curve  ID  for  relative  volume,  𝑣𝑟 = ( 𝑣
𝑣0
Remark 3 and read the beginning of the EOS section for details). 
𝜌0
𝜌 ).    (Please  see 
=
  VARIABLE   
LCID1 
LCID2 
Remarks: 
1.  The term “ambient” refers to a medium that has predetermined thermodynam-
ic  state  throughout  the  simulation.    All  “ambient”  elements  will  have  its  ther-
modynamic state reset back to this predetermined state every cycle.  If this state 
is  defined  via  the  *EOS  card,  then  this  predetermined  thermodynamic  state  is 
constant throughout the simulation.  If it is defined via the curves of the 2nd line 
for AMBTYP = 4, its thermodynamic state will vary according to these defined 
load curves.  “Ambient” elements are sometimes also referred to as “reservoir” 
elements as they may be used to simulate semi-infinite region. 
2. 
In  general,  a  thermodynamic  state  of  a  non-reacting  and  no-phase-change 
material  may  be  defined  by  2  thermodynamic  variables.    By  defining  (a)  an 
internal  energy  per  unit  reference  volume  load  curve  (or  a  temperature  load 
curve  if  using  *EOS_IDEAL_GAS)  and  (b)  a  relative  volume  load  curve,  the 
pressure as a function of time for this ambient part ID can be computed directly 
via the equation of state (*EOS_…). 
3.  A  reference  specific  volume,  𝑣0 = 1
𝜌0
,  is  the  inverse  of  a  reference  density,  𝜌0.  
The reference density is defined as the density at which the material is under a 
reference  or  nominal  state.    Please  refer  to  the  *EOS  section  for  additional  ex-
planation on this. 
4.  The internal energy per unit reference volume may be defined as 
𝑒ipv0 =
𝐶𝑣𝑇
𝑣0
. 
The  specific  internal  energy  (or  internal  energy  per  unit  mass)  is  defined  as 
𝐶𝜈𝑇. 
5.  This card does not require AET under *SECTION_SOLID or SECTION_ALE2D 
or SECTION_ALE1D card
*BOUNDARY_AMBIENT_EOS 
Purpose:    This  command  defines  the  IDs  of  2  load  curves:  (1)  internal  energy  per  unit 
reference  volume (or temperature if using *EOS_IDEAL_GAS) and (2) relative volume.  
These 2 curves completely prescribe the thermodynamic state as a function of time for 
any  ALE  or  Eulerian  part  with  an  “ambient”  type  element  formulation  (please  see 
Remark 4). 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
LCID1 
LCID2 
Type 
I 
I 
I 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION
The ambient Part ID for which the thermodynamic state is being
defined. 
Load  curve  ID  (*DEFINE_CURVE  or  *DEFINE_CURVE_FUNC-
TION) for internal energy per unit reference volume (please read
the  beginning  of  the  EOS  section  for  details).    If  *EOS_IDEAL_-
GAS is being used, this ID then refers to a temperature load curve
ID. 
Load  curve  ID  (*DEFINE_CURVE  or  *DEFINE_CURVE_FUNC-
𝜌0
TION)  for  relative  volume,  𝑣𝑟 = ( 𝑣
𝜌 ).    (Please  read  the 
=
𝑣0
beginning of the EOS section for details). 
PID 
LCID1 
LCID2 
Remarks: 
1.  The term “ambient” refers to a medium that has predetermined thermodynam-
ic state throughout the simulation.  All “ambient” parts/elements will have its 
thermodynamic state reset back to this predetermined state every cycle.  If this 
state  is  defined  via  the  *EOS  card,  then  this  predetermined  thermodynamic 
state  is  constant  throughout  the  simulation.    If  it  is  defined  via  this  card, 
*BOUNDARY_AMBIENT_EOS, then its thermodynamic state will vary accord-
ing to these defined load curves.  “Ambient” part is sometimes also referred to 
as “reservoir” part as it may be used to simulate semi-infinite region.
2. 
In  general,  a  thermodynamic  state  of  a  non-reacting  and  no-phase-change 
material  may  be  defined  by  2  thermodynamic  variables.    By  defining  (a)  an 
internal  energy  per  unit  reference  volume  load  curve  (or  a  temperature  load 
curve  if  using  *EOS_IDEAL_GAS)  and  (b)  a  relative  volume  load  curve,  the 
pressure as a function of time for this ambient part ID can be computed directly 
via the equation of state (*EOS_…). 
3.  A  reference  specific  volume,  𝑣0 = 1
𝜌0
,  is  the  inverse  of  a  reference  density,  𝜌0.  
The reference density is defined as the density at which the material is under a 
reference  or  nominal  state.    Please  refer  to  the  *EOS  section  for  additional  ex-
planation on this. 
4.  The internal energy per unit reference volume may be defined as 
𝑒ipv0 =
𝐶𝑣𝑇
𝑣0
. 
The  specific  internal  energy  (or  internal  energy  per  unit  mass)  is  defined  as 
𝐶𝜈𝑇. 
5.  This  card  is  only  to  be  used  with  “ambient”  element  type  as  defined  by  the 
parameters under the *SECTION_SOLID card: 
a)  ELFORM = 7, or  
b)  ELFORM = 11 and AET = 4, or 
c)  ELFORM = 12 and AET = 4. 
Example: 
Consider  an  ambient  ALE  part  ID  1  which  has  its  internal  energy  per  unit  reference 
volume in a load curve ID 2 and relative volume load curve ID 3: 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 
*BOUNDARY_AMBIENT_EOS 
$      PID  e/T_LCID rvol_LCID 
         1         2         3 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8
*BOUNDARY_CONVECTION_OPTION 
Available options include: 
SEGMENT 
SET 
Purpose:  Apply a convection boundary condition on a SEGMENT or SEGMENT_SET 
for a thermal analysis.  Two cards are defined for each option. 
Card 1 for SET keyword option. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
Type 
I 
Default 
none 
Card 1 for SEGMENT keyword option. 
  Card 1 
Variable 
1 
N1 
Type 
I 
2 
N2 
I 
3 
N3 
I 
4 
N4 
I 
Default 
none 
none 
none 
none 
5 
6 
7 
8 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
HLCID 
HMULT 
TLCID 
TMULT 
LOC 
Type 
I 
F 
I 
F 
Default 
none 
0. 
none 
0. 
I
VARIABLE   
DESCRIPTION
SSID 
Segment set ID, see *SET_SEGMENT. 
N1, N2, …. 
Node ID’s defining segment. 
HLCID 
Convection  heat  transfer  coefficient,  ℎ.    This  parameter  can 
reference a load curve ID  or a function ID 
.  When the reference is 
to a curve, HLCID has the following interpretation: 
GT.0:  ℎ is given as a function of time, 𝑡.  The curve consists of 
(𝑡, ℎ(𝑡)) data pairs. 
EQ.0: ℎ is a constant defined by the value HMULT. 
LT.0:  ℎ is given as a function of temperature, 𝑇𝑓𝑖𝑙𝑚.  The curve 
consists  of  (𝑇𝑓𝑖𝑙𝑚, ℎ)   data  pairs.    Enter  |HLCID|  on  the 
DEFINE_CURVE keyword.   
HMULT 
Convection heat transfer coefficient, ℎ, curve multiplier. 
TLCID 
Environment  temperature,  𝑇∞.    This  parameter  can  reference  a 
load  curve  ID    or  a  function  ID  .    When  the  reference  is  to  a 
curve, TLCID has the following interpretation: 
GT.0:  𝑇∞  is  defined  by  a  curve  indexed  by  time  consisting  of
(𝑡, 𝑇∞(𝑡)) data pairs. 
EQ.0: 𝑇∞ is a constant defined by the value TMULT. 
TMULT 
Environment temperature, 𝑇∞, curve multiplier. 
LOC 
For  a  thick  thermal  shell,  the  convection  will  be  applied  to  the
surface  identified  by  LOC.    See  parameter,  THSHEL,  on  the
*CONTROL_SHELL keyword. 
EQ.-1:  lower surface of thermal shell element 
EQ.0:  middle surface of thermal shell element 
EQ.1:  upper surface of thermal shell element 
Remarks: 
1.  A  convection  boundary  condition  is  calculated  using  𝑞 ̇′′ = ℎ(𝑇surface − 𝑇∞) 
where h is the heat transfer coefficient, and 𝑇surface − 𝑇∞ is a temperature poten-
tial.    If  h  is  a  function  of  temperature,  h  is  evaluated  at  the  average  or  “film”
temperature defined by 
 𝑇𝑓𝑖𝑙𝑚 = (𝑇surface + 𝑇∞)/2.. 
2. 
If HLCID references a DEFINE_FUNCTION, the following function arguments 
are allowed 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑍, 𝑇, 𝑇∞, 𝑡) where: 
𝑥, 𝑦, 𝑧 = segment centroid coordinates 
𝑣𝑥, 𝑣𝑦, 𝑣𝑧 = segment centroid velocity component 
𝑇 = segment centroid temperature 
𝑇∞ = environment temperature, T∞ 
𝑡 = solution time 
3. 
If TLCID references a DEFINE_FUNCTION, the following function arguments 
are allowed 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡) where: 
𝑥, 𝑦, 𝑧 = segment centroid coordinates 
𝑣𝑥, 𝑣𝑦, 𝑣𝑧 = segment centroid velocity components 
𝑡 = solution time
*BOUNDARY 
Purpose:  Define a boundary that is coupled with an external program.  Two cards are 
required for each coupled boundary 
  Card 1 
Variable 
1 
ID 
Type 
I 
2 
3 
4 
5 
6 
7 
8 
TITLE 
A70 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SET 
TYPE 
PROG 
Type 
I 
I 
I 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
ID 
ID for this coupled boundary 
TITLE 
Descriptive name for this boundary 
SET 
TYPE 
Node set ID 
Coupling type: 
EQ.1: node set with force feedback 
EQ.2: node set for multiscale spotwelds 
PROG 
Program to couple to 
EQ.1: MPP-DYNA 
Remarks: 
This  option  is  only  available  in  the  MPP  version,  and  allows  for  loose  coupling  with 
other  MPI  programs  using  a  “multiple  program”  execution  method.    Currently  it  is 
only  useful  when  linking  with  MPP-DYNA  for  the  modeling  of  multiscale  spotwelds
(type = 2, prog = 1).  See *INCLUDE_MULTISCALE_SPOTWELD for information about 
using this capability.
*BOUNDARY 
OPTION allows an optional ID to be given that applies each cyclic definition 
ID 
Purpose:  Define nodes in boundary planes for cyclic symmetry. 
These  boundary  conditions  can  be  used  to  model  a  segment  of  an  object  that  has 
rotational  symmetry  such  as  an  impeller,  i.e.,  Figure  5-1.    The  segment  boundary, 
denoted as a side 1 and side 2, may be curved or planar.  In this section, a paired list of 
points are defined on the sides that are to be joined. 
ID Card.  Additional card for ID keyword option. 
2 
3 
4 
5 
6 
7 
8 
ID 
Variable 
1 
ID 
Type 
I 
  Card 1 
Variable 
1 
XC 
Type 
F 
2 
YC 
F 
3 
ZC 
F 
HEADING 
A70 
4 
5 
6 
7 
8 
NSID1 
NSID2 
IGLOBAL 
ISORT 
I 
I 
I 
0 
I 
0 
Default 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
XC 
YC 
ZC 
x-component axis vector of axis of rotation 
y-component axis vector of axis of rotation 
z-component axis vector of axis of rotation 
NSID1 
Node set ID for first boundary (side 1, see Figure 5-1).
Conformable
Interface
Side 1
e 2
Sid
Segment
Figure  5-1.    With  axi-symmetric  cyclic  symmetry,  only  one  segment  is
modeled. 
  VARIABLE   
NSID2 
DESCRIPTION
Node  set  ID  for  second  boundary  (side  2,  see  Figure  5-1).    Each 
node  in  this  set  is  constrained  to  its  corresponding  node  in  the
first  node  set.    Node  sets  NSID1  and  NSID2  must  contain  the
same  number  of  nodal  points.    The  shape  of  the  two  surfaces
formed  by  the  two  node  sets  need  not  be  planar  but  the  shapes
should match. 
IGLOBAL 
Flag for repeating symmetry: 
EQ.0:  Axi-symmetric cyclic symmetry (default) 
EQ.1:  Repeating symmetry in planes normal to global X 
EQ.2:  Repeating symmetry in planes normal to global Y 
EQ.3:  Repeating symmetry in planes normal to global Z 
ISORT 
Set to 1 for automatic sorting of nodes in node sets.  See Remark 2.
Remarks: 
1.  Each node set should generally be boundaries of the model.
2.  Prior to version 970, it was assumed that the nodes are correctly ordered within 
each set, i.e.  the nth node in NSID1 is equivalent to the nth node in NSID2.  In 
version  970  and  later versions,  if  the  ISORT  flag  is  active,  the  nodes  in  NSID2 
are automatically sorted to achieve equivalence, so the nodes can be picked by 
the  quickest  available  method.    However,  for  axi-symmetric  cyclic  symmetry 
(IGLOBAL = 0), it is assumed that the axis passes through the origin, i.e., only 
globally defined axes of rotation are possible.
*BOUNDARY_DE_NON_REFLECTING 
Purpose:  Define a non-reflecting boundary for discrete element. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSID 
Type 
I 
Default 
none 
Remarks 
1, 2 
  VARIABLE   
DESCRIPTION
NSID 
Node set ID, see *SET_SEGMENT. 
Remarks: 
1.  Non-reflecting  boundaries  are  used  on  the  exterior  boundaries  of  an  analysis 
model  of  an  infinite  domain,  such  as  a  half-space  to  prevent  artificial  stress 
wave reflections generated at the model boundaries form reentering the model 
and contaminating the results.
Available options include: 
SEGMENT 
SET 
*BOUNDARY 
Purpose:    Apply  a  flux  boundary  condition  on  a  SEGMENT  or  SEGMENT_SET  for  a 
thermal analysis. Two or more cards are defined for each option.  History variables can 
be  associated  with  the  boundary  condition  which  will  invoke  a  call  to  a  user  defined 
boundary flux subroutine for computing the flux. 
Card 1 for SET option. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
Type 
I 
Default 
none 
Card 1 for SEGMENT option. 
  Card 1 
Variable 
1 
N1 
Type 
I 
2 
N2 
I 
3 
N3 
I 
4 
N4 
I 
Default 
none 
none 
none 
none 
5 
6 
7
Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
MLC1 
MLC2 
MLC3 
MLC4 
LOC 
NHISV 
Type 
I 
F 
Default 
none 
0. 
F 
0. 
F 
0. 
F 
0. 
I 
0 
I 
0 
Define as many cards as necessary to initialize NHISV history variables.  
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
HISV1 
HISV2 
HISV3 
HISV4 
HISV5 
HISV6 
HISV7 
HISV8 
Type 
F 
Default 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
  VARIABLE   
DESCRIPTION
SSID 
Segment set ID, see *SET_SEGMENT 
N1, N2, … 
Node IDs that define the segment
VARIABLE   
LCID 
DESCRIPTION
This  parameter  can  reference  a  load  curve  ID   or a function ID  for heat flux.  When the reference is to a curve, LCID has the
following interpretation: 
GT.0:  the  flux  is  defined  by  a  curve  consisting  of  (time, flux)
data pairs using the DEFINE_CURVE keyword.  The flux 
value applied to the nodal points is the curve value mul-
tiplied  by  the  values  MLC1,  MLC2,  MLC3,  and  MLC4, 
respectively. 
EQ.0: a  constant  flux  is  applied  to  each  node  defined  by  the
values MLC1, MLC2, MLC3, and MLC4, respectively. 
LT.0:  the 
flux 
is  defined  by  a  curve  consisting  of 
(temperature, flux)  data  pairs  using  the  DEFINE_-
CURVE  keyword.    The  flux  value  applied  to  the  nodal
points is the curve value multiplied by the values MLC1, 
MLC2,  MLC3,  and  MLC4.    Enter  |-LCID|  on  the  DE-
FINE_CURVE keyword. 
MLC1 
MLC2 
MLC3 
MLC4 
LOC 
Curve multiplier at node N1. 
Curve multiplier at node N2. 
Curve multiplier at node N3. 
Curve multiplier at node N4. 
For  a  thick  thermal  shell,  the  flux  will  be  applied  to  the  surface
identified  by  LOC.    See  parameter,  THSHEL,  on  the  *CON-
TROL_SHELL keyword. 
EQ.-1:  lower surface of thermal shell element 
EQ.0:  middle surface of thermal shell element 
EQ.1:  upper surface of thermal shell element 
NHISV 
Number of history variables associated with the flux definition: 
GT.0: A  user  defined  subroutine  will  be  called  to  compute  the
flux.  See Remark 1. 
HISV1 
HISV2 
Initial value of history variable 1 
Initial value of history variable 2
VARIABLE   
DESCRIPTION
⋮ 
⋮  
HISVn 
Initial value of history variable n, where n = NHISV 
Remarks: 
1.  The  segment  normal  has  no  bearing  on  the  flux.    A  positive  flux  transfers 
energy into the volume; a negative flux transfers energy out of the volume. 
2.  Flux can be defined by: 
a)  When  LCID = 0,  a  constant  flux  is  applied  to  each  node  defined  by  the 
values MLC1, MLC2, MLC3, and MLC4, respectively. 
b)  When  LCID > 0,  the  flux  is  defined  by  a  curve  consisting  of  (time, flux) 
data pairs using the DEFINE_CURVE keyword.  The flux value applied to 
the nodal points is the curve value multiplied by the values MLC1, MLC2, 
MLC3, and MLC4, respectively. 
c)  When  LCID < 0, 
the 
flux 
is  defined  by  a  curve  consisting  of 
(temperature, flux)  data  pairs  using  the DEFINE_CURVE  keyword.    The 
flux value applied to the nodal points is the curve value multiplied by the 
values MLC1, MLC2, MLC3, and MLC4.  Enter |LCID| on the DEFINE_-
CURVE keyword. 
d)  When NHSIV > 0, the user subroutine 
subroutine usrflux(fl, flp, ...) 
will be called to compute the heat flux (fl).  For more details see Appen-
dix S. 
e)  If  LCID  references  a  DEFINE_FUNCTION,  the  following  function  argu-
ments are allowed 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑇, 𝑇∞, 𝑡) where: 
𝑥, 𝑦, 𝑧 = segment centroid coordinates 
𝑣𝑥, 𝑣𝑦, 𝑣𝑧 = segment centroid velocity components 
𝑇 = segment centroid temperature 
𝑇∞ = environment temperature, T∞ 
𝑡 = solution time 
3.  This  keyword  is  supported  in  the  SPH  elements  to  define  the  flux  boundary 
conditions for a thermal or coupled thermal/structural analysis.  The values 𝑛1,
𝑛2,  𝑛3,  𝑛4  from  the  SPH  particles  or  segments  are  used  to  define  the  flux  seg-
ments.
*BOUNDARY_MCOL 
Purpose:  Define parameters for MCOL coupling.  The MCOL Program is a rigid body 
mechanics  program  for  modeling  the  dynamics  of  ships.    See  Remark  1  for  more 
information. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NMCOL  MXSTEP 
ETMCOL 
TSUBC  PRTMCOL
Type 
Default 
I 
2 
I 
F 
F 
F 
none 
0.0 
0.0 
none 
Remarks 
2 
Ship Card.  Include NMCOL cards, one for each ship. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RBMCOL 
MCOLFILE 
Type 
I 
Default 
A60 
none 
  VARIABLE   
DESCRIPTION
NMCOL 
Number of ships in MCOL coupling. 
MXSTEP 
Maximum  of  time  step  in  MCOL  calculation.    If  the  number  of
MCOL  time  steps  exceeds  MXSTEP,  then  LS-DYNA  will 
terminate. 
ETMCOL 
Uncoupling termination time, see Remark 2 below. 
EQ.0.0: set to LS-DYNA termination time 
TSUBC 
Time interval for MCOL subcycling. 
EQ.0.0: no subcycling
VARIABLE   
DESCRIPTION
PRTMCOL 
Time interval for output of MCOL rigid body data. 
RBMCOL 
LS-DYNA rigid body material assignment for the ship. 
MCOLFILE 
Filename containing MCOL input parameters for the ship. 
Remarks: 
1.  The  basis  for  MCOL  is  a  convolution  integral  approach  for  simulating  the 
equations of motion.  A mass and inertia tensor are required as input for each 
ship.  The masses are then augmented to include the effects of the mass of the 
surrounding  water.    A  separate  program  determines  the  various  terms  of  the 
damping/buoyancy  force  formulas  which  are  also  input  to  MCOL.    The  cou-
pling  is  accomplished  in  a  simple  manner:    at  each  time  step  LS-DYNA  com-
putes the resultant forces and moments on the MCOL rigid bodies and passes 
them to MCOL.  MCOL then updates the positions of the ships and returns the 
new rigid body locations to LS-DYNA.  A more detailed theoretical and practi-
cal description of MCOL can be found in a separate report (to appear). 
2.  After the end of the LS-DYNA/MCOL calculation, the analysis can be pursued 
using  MCOL  alone.    ETMCOL  is  the  termination  time  for  this  analysis.    If 
ETMCOL is lower than the LS-DYNA termination time, the uncoupled analysis 
will not be activated. 
3.  The  MCOL  output  is  set  to  the  files  mcolout  (ship  position)  and  mcolenergy 
(energy  breakdown).    In  LS-PrePost,  mcolout  can  be  plotted  through  the  rigid 
body time history option and MCOLENERGY
*BOUNDARY_NON_REFLECTING 
Purpose:  Define a non-reflecting boundary.  This option applies to continuum domains 
modeled with solid elements.  For geomechanical problems this option is important for 
limiting  the  spatial  extent  of  the  finite  element  mesh  and  thus  the  number  of  solid 
elements. 
4 
5 
6 
7 
8 
  Card 1 
1 
Variable 
SSID 
Type 
I 
2 
AD 
F 
3 
AS 
F 
Default 
none 
0.0 
0.0 
Remarks 
1, 2 
3 
3 
  VARIABLE   
DESCRIPTION
SSID 
AD 
Segment set ID, see *SET_SEGMENT. 
Default activation flag for dilatational waves. 
EQ.0.0: on 
NE.0.0:  off 
AS 
Default activation flag for shear waves. 
EQ.0.0: on 
NE.0.0:  off 
Remarks: 
1.  Non-reflecting boundaries defined with this keyword are only used with three-
dimensional solid elements.  Boundaries are defined as a collection of segments, 
and  segments  are  equivalent  to  element faces  on  the  boundary.    Segments  are 
defined  by  listing  the  corner  nodes  in  either  a  clockwise  or  counterclockwise 
order. 
2.  Non-reflecting  boundaries  are  used  on  the  exterior  boundaries  of  an  analysis 
model  of  an  infinite  domain,  such  as  a  half-space  to  prevent  artificial  stress 
wave reflections generated at the model boundaries form reentering the model
and  contaminating  the  results.    Internally,  LS-DYNA  computes  an  impedance 
matching  function  for  all  non-reflecting  boundary  segments  based  on  an  as-
sumption of linear material behavior.  Thus, the finite element mesh should be 
constructed  so  that  all  significant  nonlinear  behavior  is  contained  within  the 
discrete analysis model. 
3.  With  the  two  optional  switches,  the  influence  of  reflecting  waves  can  be 
studied. 
4.  During  the  dynamic  relaxation  phase  (optional),  nodes  on  non-reflecting 
segments are constrained in the normal direction.  Nodal forces associated with 
these  constraints  are  then  applied  as  external  loads  and  held  constant  in  the 
transient phase while the constraints are replaced with the impedance matching 
functions.    In  this  manner,  soil  can  be  quasi-statically  prestressed  during  the 
dynamic relaxation phase and dynamic loads (with non-reflecting boundaries) 
subsequently applied in the transient phase. 
5. 
In  explicit  analyses  this  command  has  the  side  effect  of  reducing  the  default 
value for the time step scale factor from 0.9 to 0.667.  A nonzero value of TSS-
FAC in *CONTROL_TIMESTEP will override that default.
*BOUNDARY_NON_REFLECTING_2D 
Purpose:  Define a non-reflecting boundary.  This option applies to continuum domains 
modeled  with  two-dimensional  solid  elements  in  the  xy  plane.    For  geomechanical 
problems, this option is important for limiting the size of the models. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSID 
Type 
I 
Default 
none 
Remarks 
1, 2 
  VARIABLE   
DESCRIPTION
NSID 
Node set ID, see *SET_NODE.  See Figure 5-2. 
Remarks: 
1.  Non-reflecting boundaries defined with this  keyword are only used with two-
dimensional  solid  elements  in  either  plane  strain  or  axisymmetric  geometries.  
Boundaries  are  defined  as  a  sequential  string  of  nodes  moving  counterclock-
wise around the boundary. 
2.  Non-reflecting  boundaries  are  used  on  the  exterior  boundaries  of  an  analysis 
model  of  an  infinite  domain,  such  as  a  half-space  to  prevent  artificial  stress 
wave reflections generated at the model boundaries from reentering the model 
and  contaminating  the  results.    Internally,  LS-DYNA  computes  an  impedance 
matching  function  for  all  non-reflecting  boundary  segments  based  on  an  as-
sumption of linear material behavior.  Thus, the finite element mesh should be 
constructed  so  that  all  significant  nonlinear  behavior  in  contained  within  the 
discrete analysis model.
Define the nodes k, k+1, k+2, ...,
k+n while moving counterclockwise
around the boundary.
k+2
k+1
k+n
Figure    5-2.    When  defining  a  transmitting  boundary  in  2D  define  the  node
numbers in the node set in consecutive order while moving counterclockwise
around the boundary.
*BOUNDARY_PAP 
Purpose:    Define  pressure  boundary  conditions  for  pore  air  flow  calculation,  e.g.    at 
structure surface exposed to atmospheric pressure.   
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SEGID 
LCID 
CMULT 
CVMASS 
BLOCK 
TBIRTH 
TDEATH 
CVRPER 
Type 
I 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
0.0 
0.0 
1.e20 
1.0 
Remark 
1, 2 
3 
  VARIABLE   
DESCRIPTION
SEGID 
Segment set ID 
LCID 
Load curve giving pore air pressure vs.  time. 
EQ.0: constant pressure assumed equal to CMULT 
CMULT 
Factor on curve or constant pressure head if LCID = 0 
CVMASS 
Initial mass of a control volume next to the segment set SETID 
BLOCK 
Contact blockage effect, 
EQ.0: When  all  segments  in  SEGID  are  subject  to  the  pressure
defined by LCID and CMULT; 
EQ.1: When  only  elements  in  SEGID  not  involved  in  contact 
are subject to the pressure defined by LCID and CMULT.
TBIRTH 
Time at which boundary condition becomes active 
TDEATH 
Time at which boundary condition becomes inactive 
CVRPER 
Permeability factor of cover material, where cover refers to a shell
layer coating the surface of the solid.  Default value is 1.0 when it
is not defined.  See Remark 3 below. 
0.0 ≤ CVRPER ≤ 1.0
Control Volume
SEGID
Segment ID for the part
of the boundary through
which air flows to and from
the control volume. 
Sample
Figure 5-3.  Air flows between the control volume and the sample.  CVMASS
specifies  the  control  volume’s  initial  mass,  and  CVMULT  sets  the  initial
pressure. 
Remarks: 
1.  All structure surfaces subject to specified pressure have to be defined. 
2.  A  non-zero  CVMASS,  together  with  a  non-zero  CMULT  and  an  un-defined 
LCID, can be used to simulate air mass transfer between a control volume and a 
test  specimen  containing  pore  air.    The  control  volume  is  assumed  to  have  a 
fixed  volume,  and  have  initial  pressure  of  CMULT  and  initial  mass  of 
CVMASS.  Air mass transfer happens between control volume and its neighbor-
ing specimen.  Such mass transfer results in pressure change in control volume 
and test specimen. 
3.  CVRPER allows users to model the porosity properties of the cover material.  If 
SEGID is covered by a material of very low permeability (e.g., coated fabric), it 
is  appropriate  to  set  CVRPER = 0.    In  this  case,  Pc,  the  pressure  calculated  as-
suming  no  boundary  condition,  is  applied  to  SEGID.    If  SEGID  is  not  covered 
by any material, it is appropriate to set CVRPER = 1, the default value.  In this 
case,  the  applied  pressure  becomes  Pb,  the  boundary  pressure  determined  by 
CMULT and LCID.
*BOUNDARY_PORE_FLUID_OPTION 
Available options include: 
PART 
SET 
Purpose:    Define  parts  that  contain  pore  fluid.    Defaults  are  given  on  *CONTROL_-
PORE_FLUID. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
P(S)ID  WTABLE 
PF_RHO 
ATYPE 
PF_BULK
ACURVE  WTCUR 
SUCLIM 
Type 
I 
Default 
none 
F 
* 
F 
* 
I 
* 
F 
* 
I 
0 
I 
0 
F 
0. 
*  Defaults are taken from *CONTROL_PORE_FLUID 
  VARIABLE   
PID, PSID 
DESCRIPTION
Part  ID  (PID)  or  Part  set  ID,  see  *PART  and  *SET_PART.    All 
elements within the part must lie below the water table. 
WTABLE 
Z-coordinate at which pore pressure = 0 (water table)   
PF_RHO 
Density of pore water in soil skeleton: 
EQ.0: Default  density  specified  on  *CONTROL_PORE_FLUID 
card is used. 
ATYPE 
Analysis type for Parts: 
EQ.0: Default to value specified on *CONTROL_PORE_FLUID
EQ.1: Undrained analysis 
EQ.2: Drained analysis 
EQ.3: Time dependent consolidation (coupled) 
EQ.4: Consolidate to steady state (uncoupled) 
EQ.5: Drained in dynamic relaxation, undrained in transient
VARIABLE   
DESCRIPTION
PF_BULK 
Bulk modulus of pore fluid: 
EQ.0: Default to value specified on *CONTROL_PORE_FLUID
ACURVE 
Curve of analysis type vs time  
WTCUR 
Curve of water table (z-coordinate) vs time   
SUCLIM 
Suction  limit  (defined  in  head,  i.e.    length  units).    Must  not  be
negative.  See remarks. 
Remarks: 
This card must be present for all parts having pore water. 
The density on this card is used only to calculate pressure head.  To ensure the correct 
gravity loading, the density of the soil material should be increased to include the mass 
associated with the pore water. 
The  y-axis  values  of  the  curve  of  analysis  type  vs  time  can  only  be  1,  2  or  3.    During 
dynamic relaxation, the analysis type will be taken from the first value on the curve   
The  default  for  SUCLIM  is  zero,  meaning  that  the  pore  fluid  cannot  generate  suction.  
To allow unlimited suction, set this parameter to a large positive number.
*BOUNDARY_PRECRACK 
Purpose:  Define pre-cracks in XFEM shell formulations 52 or 54 for purposes of fracture 
analysis.   
4 
5 
6 
7 
8 
  Card 1 
1 
2 
Variable 
PID 
CTYPE 
Type 
I 
Default 
I 
1 
3 
NP 
I 
Precrack Point Cards.  Include NP cards, one for each point in the pre-crack. 
4 
5 
6 
7 
8 
1 
X 
F 
2 
Y 
F 
3 
Z 
F 
  Card 2 
Variable 
Type 
Default 
  VARIABLE   
DESCRIPTION
PID 
Part ID where the pre-crack is located 
CTYPE 
Type of pre-crack: 
EQ.1: straight line 
NP 
Number of points defining the pre-crack 
X, Y, Z 
Coordinates of the points defining the pre-crack
*BOUNDARY_PRESCRIBED_ACCELEROMETER_RIGID 
Purpose:    Prescribe  the  motion  of  a  rigid  body  based  on  experimental  data  obtained 
from accelerometers affixed to the rigid body. 
Note: This feature is available starting with LS-DYNA 971R3. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
SOLV 
Type 
I 
Default 
none 
I 
1 
Accelerometer  Cards.    Define  one  card  for  each  accelerometer  affixed  to  the  rigid 
body.    Input  is  terminated  when  a  “*”  card  is  found.    A  minimum  of  three 
accelerometers are required . 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID 
CID 
LCIDX 
LCIDY 
LCIDZ 
Type 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
PID 
Part ID for rigid body whose motion is prescribed. 
SOLV 
Solver type: 
EQ.1: Gaussian elimination (default), 
EQ.2: linear regression 
NID 
CID 
Node ID corresponding to the location of the accelerometer. 
the
Coordinate  system 
accelerometer’s 
*DEFINE_COORDINATE_-
NODES).  All nodes must reside on the same part.  Set FLAG = 1.
the  orientation  of 
ID  describing 
local  axes 
(see
VARIABLE   
DESCRIPTION
Load  curve  ID  containing  the  local  x-acceleration  time  history 
from the accelerometer. 
Load  curve  ID  containing  the  local  y-acceleration  time  history 
from the accelerometer. 
Load  curve  ID  containing  the  local  z-acceleration  time  history 
from the accelerometer. 
LCIDX 
LCIDY 
LCIDZ 
Remarks: 
1.  Acceleration  time  histories  from  a  minimum  of  three  accelerometers  each 
providing output from three channels are required.  Load curves must have the 
same number of points and data must be uniformly spaced. 
2.  Local axes of the accelerometers must be orthogonal.
*BOUNDARY_PRESCRIBED_FINAL_GEOMETRY 
The final displaced geometry for a subset of nodal points is defined.  The nodes of this 
subset  are  displaced  from  their  initial  positions  specified  in  the  *NODE  input  to  the 
final geometry along a straight line trajectory.  A load curve defines a scale factor as a 
function  of  time  that  is  bounded  between  zero  and  unity  corresponding  to  the  initial 
and final geometry, respectively.  A unique load curve can be specified for each node, 
or  a  default  load  curve  can  apply  to  all  nodes.      The  external  work  generated  by  the 
displacement field is included in the energy ratio calculation for the glstat file. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BPFGID 
LCIDF 
DEATHD 
Type 
Default 
I 
0 
I 
0 
F 
infinity 
Node Cards.  The next “*” keyword card terminates this input.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
NID 
Type 
I 
X 
F 
Default 
none 
0. 
Y 
F 
0. 
Z 
F 
0. 
LCID 
DEATH 
I 
F 
LCIDF 
infinity 
  VARIABLE   
DESCRIPTION
BPFGID 
ID for this set of imposed boundary conditions   
LCIDF 
Default load curve ID.  This curve varies between zero and unity.  
DEATHD 
Default death time.  At this time the prescribed motion is inactive
and the nodal point is allowed to move freely.   
NID 
Node ID for which the final position is defined.  Nodes defined in 
this section must also appear under the *NODE input.  
X 
x-coordinate of final geometry
VARIABLE   
DESCRIPTION
Y 
Z 
y-coordinate of final geometry 
z-coordinate of final geometry 
LCID 
Load curve ID.  If zero the default curve ID, LCIDF, is used. 
DEATH 
Death time.  If zero the default value, DEATHD, is used.
*BOUNDARY_PRESCRIBED_MOTION_OPTION1_{OPTION2} 
Available options for OPTION1 include: 
NODE 
SET 
SET_BOX 
SET_SEGMENT 
RIGID 
RIGID_LOCAL 
SET_LINE 
OPTION2 allows an optional ID to be given that applies either to the single node, node 
set or a rigid body. 
ID 
If a heading is defined with the ID, then the ID with the heading will be written at the 
beginning of the ASCII file, bndout. 
Purpose:  Define an imposed nodal motion (velocity, acceleration, or displacement) on a 
node  or  a  set  of  nodes.    Also  velocities  and  displacements  can  be  imposed  on  rigid 
bodies.    If  the  local  option  is  active  the  motion  is  prescribed  with  respect  to  the  local 
coordinate  system  for  the  rigid  body  .  
Translational  nodal  velocity  and  acceleration  specifications  for  rigid  body  nodes  are 
allowed  and  are  applied  as  described  at  the  end  of  this  section.    For  nodes  on  rigid 
bodies  use  the  NODE  option.    Do  not  use  the  NODE  option  in  r-adaptive  problems 
since the node ID's may change during the adaptive step. 
The  SET_LINE  option  allows  a  node  set  to  be  generated  including  existing  nodes  and 
new nodes created from h-adaptive mesh refinement along the straight line connecting 
two specified nodes to be included in prescribed boundary conditions.
HEADING 
A70 
5 
SF 
F 
*BOUNDARY 
*BOUNDARY_PRESCRIBED_MOTION 
ID Card.  Additional card for ID keyword option.  
2 
3 
4 
5 
6 
7 
8 
ID 
Variable 
1 
ID 
Type 
I 
  Card 1 
1 
2 
3 
4 
Variable 
typeID 
DOF 
VAD 
LCID 
Type 
I 
I 
Default 
none 
none 
I 
0 
I 
none 
1. 
6 
7 
8 
VID 
DEATH 
BIRTH 
I 
0 
F 
F 
1028 
0.0 
For the SET_BOX keyword option, define the following additional card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BOXID 
TOFFSET  LCBCHK 
Type 
I 
Default 
none 
I 
0 
I 
0 
Additional  card  that  is  expected  if  DOF = 9,  10,  11  or  VAD = 4  on  the  first  card; 
otherwise skip this card. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  OFFSET1  OFFSET2 
MRB 
NODE1 
NODE2 
Type 
F 
Default 
0. 
F 
0. 
I 
0 
I 
0 
I
For the SET_LINE keyword option, define the following additional card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NBEG 
NEND 
Type 
I 
I 
Default 
none 
none 
  VARIABLE   
DESCRIPTION
ID 
Optional PRESCRIBED MOTION set ID to which this node, node
set, segment set or rigid body belongs.  This ID does not need to
be unique. 
HEADING 
An  optional  descriptor  for  the  given  ID  that  will  be  written  into
the d3hsp file and the bndout file. 
typeID 
Node  ID  (NID  in  *NODE),  nodal  set  ID  (SID  in  *SET_NODE), 
segment set ID (SID in *SET_SEGMENT, see DOF = 12) or part ID 
(PID in *PART) for a rigid body. 
DOF 
Applicable degrees-of-freedom: 
EQ.1: 
EQ.2: 
EQ.3: 
EQ.4: 
EQ.-4: 
EQ.5: 
EQ.6: 
EQ.7: 
EQ.8: 
𝑥-translational degree-of-freedom, 
𝑦-translational degree-of-freedom, 
𝑧-translational degree-of-freedom, 
translational  motion  in  direction  given  by  the  VID.
Movement on plane normal to the vector is permitted.
translational  motion  in  direction  given  by  the  VID. 
Movement on plane normal to the vector is not permit-
ted.  This option does not apply to rigid bodies. 
𝑥-rotational degree-of-freedom, 
𝑦-rotational degree-of-freedom, 
𝑧-rotational degree-of-freedom, 
rotational motion about a vector parallel to vector VID. 
Rotation about the normal axes is permitted. 
EQ.-8:  rotational motion about a vector parallel to vector VID.
Rotation about the normal axes is not permitted.  This
VARIABLE   
DESCRIPTION
option does not apply to rigid bodies. 
EQ.9: 
𝑦/𝑧 degrees-of-freedom for node rotating about the 𝑥-
axis  at  location  (OFFSET1,  OFFSET2)  in  the  𝑦𝑧-plane, 
point (𝑦, 𝑧).  Radial motion is NOT permitted.  Not ap-
plicable to rigid bodies. 
EQ.-9:  𝑦/𝑧 degrees-of-freedom for node rotating about the 𝑥-
axis  at  location  (OFFSET1,  OFFSET2)  in  the  𝑦𝑧-plane, 
point (𝑦, 𝑧).  Radial motion is permitted.  Not applica-
ble to rigid bodies. 
EQ.10:  𝑧/𝑥 degrees-of-freedom for node rotating about the 𝑦-
axis  at  location  (OFFSET1,  OFFSET2)  in  the  𝑧𝑥-plane, 
point (𝑧, 𝑥).  Radial motion is NOT permitted.  Not ap-
plicable to rigid bodies. 
EQ.-10:  𝑧/𝑥 degrees-of-freedom for node rotating about the 𝑦-
axis  at  location  (OFFSET1,  OFFSET2)  in  the  𝑧𝑥-plane, 
point (𝑧, 𝑥).  Radial motion is permitted.  Not applica-
ble to rigid bodies. 
EQ.11:  𝑥/𝑦 degrees-of-freedom for node rotating about the z-
axis  at  location  (OFFSET1,  OFFSET2)  in  the  𝑥𝑦-plane, 
point (𝑥, 𝑦).  Radial motion is NOT permitted.  Not ap-
plicable to rigid bodies. 
EQ.-11:  𝑥/𝑦 degrees-of-freedom for node rotating about the 𝑧-
axis  at  location  (OFFSET1,  OFFSET2)  in  the  𝑥𝑦-plane, 
point (𝑥, 𝑦).  Radial motion is permitted.  Not applica-
ble to rigid bodies. 
EQ.12:  translational motion in direction given by the normals
to the segments defined by the set typeID.   
VAD 
Velocity/Acceleration/Displacement flag: 
EQ.0: velocity (rigid bodies and nodes), 
EQ.1: acceleration (rigid bodies and nodes), 
EQ.2: displacement (rigid bodies and nodes). 
EQ.3: velocity versus displacement (rigid bodies only) 
EQ.4: relative displacement (rigid bodies only)
VARIABLE   
LCID 
DESCRIPTION
Curve ID or function ID to describe motion value versus time, see
*DEFINE_CURVE, 
*DE-
FINE_FUNCTION.    If  LCID  refers  to  *DEFINE_FUNCTION,  the 
function  can  have  only  time  as  an  argument,  e.g.,  𝑓 (𝑡) = 10.0 × 𝑡. 
See BIRTH below. 
*DEFINE_CURVE_FUNCTION,  or 
SF 
VID 
Load curve scale factor.  (default = 1.0) 
Vector ID for DOF values of 4 or 8, see *DEFINE_VECTOR.  The 
direction of this vector is not updated with time. 
DEATH 
Time imposed motion/constraint is removed: 
EQ.0.0: default set to 1028 
BIRTH 
BOXID 
LCBCHK 
Time  that  the  imposed  motion/constraint  is  activated.    The 
prescribed  motion  begins  acting  at  time = BIRTH  but  from  the 
zero  abscissa  value  of  the  curve  or  function  (*DEFINE_FUNC-
TION).    In  other  words,  the  abscissae  are  shifted  by  an  amount 
BIRTH,  i.e.,  it  has  the  same  effect  as  setting  OFFA = BIRTH  in 
*DEFINE_CURVE.    Warning:    BIRTH  is  ignored  if  the  LCID  is 
defined as a function, i.e., *DEFINE_CURVE_FUNCTION.   
A box ID defining a box region in space in which the constraint is
activated.    Only  the  nodes  falling  inside  the  box  will  be  applied
the  prescribed  motion.    If  LCBCHK  is  not  defined,  the  box
volume is reevaluated every time step to determine the nodes for
which  the  prescribed  motion  is  active.    This  reevaluation  of  the
volume is referred to as a “box-check”. 
Optional  load  curve  allowing  more  flexible  and  efficient  use  of
SET_BOX option.  Instead of performing box-check at every time 
step,  discrete  box-check  times  could  be  given  as  𝑥-values  of 
LCBCHK.    LCBCHK’s  𝑦-values  specify  corresponding  death 
times.  For example, a curve with points (20, 30) and (50, 70) will
result  in  two  box  checks.    The  first  will  occur  at  20,  and  the
prescribed motion will be active from 20 to 30.   The second will 
occur  at  50,  and  the  prescribed  motion  will  be  active  from  50  to
70.  A 𝑦-value of “0” means the prescribed motion will stay active
until next box-check.  For example, an additional 3rd point of (90, 
0) will lead to another box-check at 90, and the prescribed motion 
will be active from 90 until the end of the simulation.
VARIABLE   
DESCRIPTION
TOFFSET 
Time offset flag for the SET_BOX option: 
EQ.1: the time value of the load curve, LCID, will be offset by
the time when the node enters the box, 
EQ.0: no time offset is applied to LCID 
OFFSET1 
Offset for DOF types 9-11 (𝑦, 𝑧, 𝑥 direction) 
OFFSET2 
Offset for DOF types 9-11 (𝑧, 𝑥, 𝑦 direction) 
MRB 
Master rigid body for measuring the relative displacement. 
NODE1 
Optional orientation node, n1, for relative displacement 
NODE2 
Optional orientation node, n2, for relative displacement 
Node ID of a starting node. 
Node  ID  of  an  ending  node.    All  existing  nodes  and  new  nodes
generated  by  h-adaptive  mesh  refinement  along  the  straight  line 
connecting  NBEG  and  NEND  will  be  included  in  the  prescribed
boundary motions. 
NBEG 
NEND 
Remarks: 
When DOF = 5, 6, 7, or 8, nodal rotational degrees-of-freedom are prescribed in the case 
of deformable nodes (OPTION1 = NODE or SET) whereas body rotations are prescribed 
in the case of a rigid body (OPTION1 = RIGID).  In the case of a rigid body, the axis of 
prescribed  rotation  always  passes  through  the  body's  center  of  mass.    For  |DOF| = 8, 
the axis of the prescribed rotation is parallel to vector VID.  To prescribe a body rotation 
of a set of deformable nodes, with the axis of rotation parallel to global axes 𝑥, 𝑦, or 𝑧, 
use  OPTION1 = SET  with  |DOF| = 9,  10,  or  11,  respectively.    The  load  curve  scale 
factor can be used for simple modifications or unit adjustments. 
The relative displacement can be measured in either of two ways: 
1.  Along a straight line between the mass centers of the rigid bodies, 
2.  Along a vector beginning at node 𝑛1 and terminating at node 𝑛2. 
With  option  1,  a  positive  displacement  will  move  the  rigid  bodies  further  apart,  and, 
likewise a negative motion will move the rigid bodies closer together.  The mass centers 
of the rigid bodies must not be coincident when this option is used.  With option 2 the 
relative  displacement  is  measured  along  the  vector,  and  the  rigid  bodies  may  be
coincident.  Note that the motion of the master rigid body is not directly affected by this 
option, i.e., no forces are generated on the master rigid body. 
The activation time, BIRTH, is the time during the solution that the constraint begins to 
act.    Until  this  time,  the  prescribed  motion  card  is  ignored.    The  function  value  of  the 
load curves will  be evaluated at the offset time given by the difference of the solution 
time and BIRTH, i.e., (solution time-BIRTH).  Relative displacements that occur prior to 
reaching  BIRTH  are  ignored.    Only  relative  displacements  that  occur  after  BIRTH  are 
prescribed. 
When  the  constrained  node  is  on  a  rigid  body,  the  translational  motion  is  imposed 
without  altering  the  angular  velocity  of  the  rigid  body  by  calculating  the  appropriate 
translational velocity for the center of mass of the rigid body using the equation: 
𝐯cm = 𝐯node − 𝛚 × (𝐱cm − 𝐱node) 
where 𝐯𝑐𝑚 is the velocity of the center of mass, 𝐯node is the specified nodal velocity, 𝛚 is 
the angular velocity of the rigid body, 𝐱cm is the current coordinate of the mass center, 
and 𝐱node is the current coordinate of the nodal point.  Extreme care must be used when 
prescribing motion of a rigid body node.  Typically, for nodes on a given rigid body, the 
motion  of  no  more  than  one  node  should  be  prescribed  or  unexpected  results  may  be 
obtained. 
When the RIGID option is used to prescribe rotation of a rigid body, the axis of rotation 
will always be shifted such that it passes through the center-of-mass of the rigid body.  
By using *PART_INERTIA or *CONSTRAINED_NODAL_RIGID_BODY_INERTIA, one 
can override the internally-calculated location of the center-of-mass. 
When  the  RIGID_LOCAL  option  is  invoked,  the  orientation  of  the  local  coordinate 
system rotates with time in accordance with rotation of the rigid body. 
Angular displacements are applied in an incremental fashion hence it is not possible to 
correctly prescribe a successive set of rotations about multiple axes.  In light of this the 
command *BOUNDARY_PRESCRIBED_ORIENTATION_RIGID should be used for the 
purpose of prescribing the general orientation of a rigid body. 
Example: 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *BOUNDARY_PRESCRIBED_MOTION_SET 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  A set of nodes is given a prescribed translational velocity in the 
$  x-direction according to a specified vel-time curve (which is scaled). 
$ 
*BOUNDARY_PRESCRIBED_MOTION_SET 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8
$     nsid       dof       vad      lcid        sf       vid     death 
         4         1         0         8       2.0 
$ 
$     nsid = 4    nodal set ID number, requires a *SET_NODE_option 
$      dof = 1    motion is in x-translation 
$      vad = 0    motion prescribed is velocity 
$     lcid = 8    velocity follows load curve 8, requires a *DEFINE_CURVE 
$       sf = 2.0  velocity specified by load curve is scaled by 2.0 
$      vid        not used in this example 
$    death        use default (essentially no death time for the motion) 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *BOUNDARY_PRESCRIBED_MOTION_RIGID 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  A rigid body is given a prescribed rotational displacement about the 
$  z-axis according to a specified displacement-time curve. 
$ 
*BOUNDARY_PRESCRIBED_MOTION_RIGID 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      pid       dof       vad      lcid        sf       vid     death 
        84         7         2         9                          14.0 
$ 
$      pid = 84   apply motion to part number 84 
$      dof = 7    rotation is prescribed about the z-axis 
$      vad = 2    the prescribed motion is displacement (angular) 
$     lcid = 9    rotation follows load curve 9, requires a *DEFINE_CURVE 
$                     (rotation should be in radians) 
$       sf        use default (sf = 1.0) 
$      vid        not used in this example 
$    death = 14   prescribed motion is removed at 14 ms (assuming time is in ms) 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
SET_LINE option: 
Referring to Figure 5-4 and a partial keyword example below, a flat plate is being pulled 
along  one  edge  while  the  opposite  edge  is  fully  constrained.    All  four  existing  nodes 
and  new  nodes  created  from  h-adaptive  mesh  refinement  along  the  straight  line 
connecting nodes 98 and 105 will be included in a node set ID 122, which is subjected to 
a velocity boundary condition defined by load curve ID 2.  From the deformed shape, it 
is evident all nodes are pulled equally according to the boundary condition. 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
*BOUNDARY_PRESCRIBED_MOTION_SET_LINE 
$#    nsid       dof       vad      lcid        sf       vid     death     birth 
       122         3         0         2 
$     NBEG     NEND 
        98      105 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
*DEFINE_CURVE
0.0              &velo 
            &endtime              &velo 
              1000.0              &velo 
Revision Information: 
SET_LINE option is available starting in Revision 109996 for both SMP and MPP.
All nodes fixed 
along this edge
Undeformed mesh
X Y
Node 98
Node 105
All existing nodes along the 
straight line connecting nodes 98 
and 105 are automatically included 
in the displacement boundary.
A displacement boundary condition
Node 105
Deformed mesh
Node 98
New nodes created from 
adaptive refinement along the 
straight line connecting nodes 
98 and 105 are also included 
in the displacement boundary.
Figure 5-4.  The SET_LINE option usage.
*BOUNDARY_PRESCRIBED_ORIENTATION_RIGID_OPTION1_{OPTION2} 
Available options OPTION1 include: 
DIRCOS 
ANGLES 
EULERP 
VECTOR 
OPTION2 allows an optional ID: 
ID 
The defined ID can be referred to by *SENSOR_CONTROL. 
Purpose:  Prescribe the orientation of rigid body as a function of time. 
Card Formats: 
ID Card.  Optional card for ID keyword option.  
ID 
Variable 
1 
ID 
Type 
I 
2 
3 
4 
5 
6 
7 
8 
HEADING 
A70 
Card 1 is common to all orientation methods. 
Cards 2 to 3 are unique for each orientation method. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PIDB 
PIDA 
INTRP 
BIRTH 
DEATH 
TOFFSET 
Type 
I 
Default 
none 
I 
0 
I 
1 
F 
0. 
F 
1020 
I
VARIABLE   
ID 
DESCRIPTION
Optional  ID  for  PRESCRIBED  ORIENTATION  that  can  be
referred  to  by  *SENSOR_CONTROL.    When  not  defined,  the
sequential definition order will be used as ID when referred to by
*SENSOR_CONTROL.   
HEADING 
An optional descriptor for the given ID. 
PIDA 
Part  ID  for  rigid  body  A.    If  zero  then  orientation  of  PIDB  is
performed with respect to the global reference frame. 
INTRP 
Interpolation method used on time history curves: 
EQ.1: linear interpolation (default) 
EQ.2: cubic  spline 
development) 
interpolation 
(experimental  –  under 
BIRTH 
DEATH 
Prior to this time the body moves freely under the action of other
agents. 
The body is freed at this time and subsequently allowed to move
under the action of other agents. 
TOFFSET 
Time offset flag: 
EQ.1: The  time  value  of  all  load  curves  will  be  offset  by  the 
birth time. 
EQ.0: No time offset is applied. 
Cosine Card 1.  Additional card for DIRCOS option.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCIDC11  LCIDC12  LCIDC13  LCIDC21  LCIDC22  LCIDC23  LCIDC31  LCIDC32 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none
Cosine Card 2.  Additional card for DIRCOS option.  
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCIDC33 
Type 
I 
Default 
none 
  VARIABLE   
LCIDCij 
DESCRIPTION
Load  curve  ID  specifying  direction  cosine  𝐶𝑖𝑗  as  a  function  of 
time. 𝐶𝑖𝑗 is defined as: 
𝐶𝑖𝑗 = 𝐚𝑖 ⋅ 𝐛𝑗 
where  the {𝒂𝑖}  are  mutually  perpendicular  unit  vectors  fixed  in
PIDA and the {𝒃𝑗} are mutually perpendicular unit vectors fixed
in  PIDB.    If  PIDA = 0  then  the  {𝒂𝑖}  are  unit  vectors  aligned  with 
the global 𝑥, 𝑦, and 𝑧.  See Remark 1. 
Angles Card.  Additional card for ANGLES option. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCIDQ1 
LCIDQ2 
LCIDQ3 
ISEQ 
ISHFT 
BODY 
Type 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
I 
1 
I 
0 
  VARIABLE   
LCIDQi 
ISEQ 
DESCRIPTION 
Load  curve  ID  specifying  the  orientation  angle  𝑞𝑖  in  radians  as  a 
function of time.  See Remark 1. 
Specifies the sequence in which the rotations are performed.  In this 
first set of sequences three unique axes are involved.  This sequence 
is associated with what are commonly called Cardan or Tait-Bryan 
angles.  All angles are in units of radians.  Whether these rotations are 
intrinsic or extrinsic is determined by the BODY field.
EQ.123:  The first rotation is performed about the 𝑥 axis through 
an  angle  of 𝑞1,  the  second  about  the 𝑦  axis  through  an 
angle  of 𝑞2,  and  the  third  about  the  𝑧  axis  through  an 
angle of 𝑞3. 
EQ.231:  The first rotation is performed about the 𝑦 axis through 
an  angle  of 𝑞1,  the  second  about  the  𝑧  axis  through  an 
angle  of 𝑞2,  and  the  third  about  the  𝑥  axis  through  an 
angle of 𝑞3. 
EQ.312:  The first rotation is performed about the 𝑧 axis through 
an  angle  of 𝑞1,  the  second  about  the  𝑥  axis  through  an 
angle  of 𝑞2,  and  the  third  about  the  𝑦  axis  through  an 
angle of 𝑞3. 
EQ.132:  The first rotation is performed about the 𝑥 axis through 
an  angle  of 𝑞1,  the  second  about  the  𝑧  axis  through  an 
angle  of 𝑞2,  and  the  third  about  the  𝑦  axis  through  an 
angle of 𝑞3. 
EQ.213:  The first rotation is performed about the 𝑦 axis through 
an  angle  of 𝑞1,  the  second  about  the  𝑥  axis  through  an 
angle  of 𝑞2,  and  the  third  about  the  𝑧  axis  through  an 
angle of 𝑞3. 
EQ.321:  The first rotation is performed about the 𝑧 axis through 
an  angle  of 𝑞1,  the  second  about  the 𝑦  axis  through  an 
angle  of 𝑞2,  and  the  third  about  the  𝑧  axis  through  an 
angle of 𝑞3. 
The  second  set  of  sequences  involve  only  two  unique  axes  where 
the  first  and  third  are  repeated.    This  sequence  is  associated  with 
what are commonly called Euler angles. 
EQ.121:  the  first  rotation  is  performed  about  the  𝑥  axis  through 
an  angle  of 𝑞1,  the  second  about  the 𝑦  axis  through  an 
angle  of 𝑞2,  and  the  third  about  the  𝑥  axis  through  an 
angle of 𝑞3. 
EQ.131:  The first rotation is performed about the 𝑥 axis through 
an  angle  of 𝑞1,  the  second  about  the 𝑧  axis  through  an 
angle  of 𝑞2,  and  the  third  about  the  𝑥  axis  through  an 
angle of 𝑞3. 
EQ.212:  The first rotation is performed about the 𝑦 axis through 
an  angle  of 𝑞1,  the  second  about  the 𝑥  axis  through  an 
angle  of 𝑞2,  and  the  third  about  the  𝑦  axis  through  an 
angle of 𝑞3. 
EQ.232:  The first rotation is performed about the 𝑦 axis through
an  angle  of 𝑞1,  the  second  about  the 𝑧  axis  through  an 
angle  of 𝑞2,  and  the  third  about  the  𝑦  axis  through  an 
angle of 𝑞3. 
EQ.313:  The first rotation is performed about the 𝑧 axis through 
an  angle  of 𝑞1,  the  second  about  the 𝑥  axis  through  an 
angle  of 𝑞2,  and  the  third  about  the  𝑧  axis  through  an 
angle of 𝑞3. 
EQ.323:  The first rotation is performed about the 𝑧 axis through 
an  angle  of 𝑞1,  the  second  about  the 𝑦  axis  through  an 
angle  of 𝑞2,  and  the  third  about  the  𝑧  axis  through  an 
angle of 𝑞3. 
ISHFT 
Angle shift. 
EQ.1: Angle curves are unaltered. 
EQ.2: Shifts  angle  data  in  the  LCIDQi  curves  as  necessary  to 
eliminate  discontinuities.    If  angles  are  confined  to  the 
range [−𝜋, 𝜋] and the data contains excursions exceeding 
𝜋 then set ISHFT = 2. 
BODY 
Reference axes. 
EQ.0: Rotations  are  performed  about  axes  fixed  in  PIDA 
(extrinsic rotation, default). 
EQ.1: Rotations are performed about axes fixed in PIDB (intrinsic 
rotation). 
Euler Parameter Card.  Additional card for EULERP option.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCIDE1 
LCIDE2 
LCIDE3 
LCIDE4 
Type 
I 
I 
I 
I 
Default 
none 
none 
none 
none
VARIABLE   
LCIDEi 
DESCRIPTION
Load curve ID specifying Euler parameter 𝑒𝑖 as a function of time. 
The Euler parameters are defined as follows.  See Remark 1. 
𝜀𝑖 = 𝜺 ⋅ 𝒂𝑖 = 𝜺 ⋅ 𝒃𝑖,
(𝑖 = 1, 2, 3) 
𝜀4 = cos (
) 
where  𝜺  is  the  Euler  vector, {𝒂𝑖}  and  {𝒃𝑖}  are  dextral  sets  of  unit 
vectors fixed in PIDA and PIDB, respectively, and 𝜃 (in radians) is 
associated with the rotation of PIDB in PIDA about Euler vector.
If  PIDA = 0  then  the  {𝒂𝑖}  are  unit  vectors  aligned,  respectively, 
with the global 𝑥, 𝑦, and 𝑧 axes. 
2)𝒏 and 𝜀4 = cos(𝜃
The Euler parameters are defined as 𝜺 = sin(𝜃
2), respectively.  Here 𝒏 
is a unit vector defining the axis of rotation, and 𝜃 is the angle with which the rotation 
2 =
occurs, and consequently the four parameters are subjected to the condition  𝛆𝑇𝛆 + 𝜀4
1.  It is therefore recommended that the control points of the curves already fulfil this or 
else  LS-DYNA  will  internally  normalize  these  values.    From  the  Euler  parameters  at 
time  𝑡,  a  unique  rotation  matrix  𝑸𝑡  is  computed  that  is  used  to  determine  the  total 
orientation 𝑸.  The rotation is performed with respect to the reference state 𝑸0 given by 
the Euler parameters at time 0.  In general, 𝑸0 ≠ 𝑰 and the rotation of the rigid body is 
𝑇.  If the parameters are initially 𝜺 = 𝟎 and 𝜀4 = 1, then the reference 
given by 𝑸 = 𝑸𝑡𝑸0
state is 𝑸0 = 𝑰 and 𝑸 = 𝑸𝑡 defines the orientation of the rigid body.  
For  a  nonzero  PIDA,  the  rotation  matrix  𝑸  as  defined  above  is  expressed  in  a  system 
that is fixed in rigid body A.  If this system is denoted 𝑹𝑡 at time 𝑡, and assuming 𝑹0 =
𝑰, the orientation with respect to a global system is 𝑹𝑸.  
Vector Card.  Additional card for VECTOR option.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCIDV1 
LCIDV2 
LCIDV3 
LCIDS 
VALSPIN 
Type 
I 
I 
I 
Default 
none 
none 
none 
I 
0 
F 
0.
VARIABLE   
LCIDVi 
DESCRIPTION
Load  curve  ID  specifying  the  vector  measure  number  𝑣𝑖  as  a 
function  of  time.    The  vector  measure  numbers  are  defined  as
follows.  See Remark 1. 
𝑣𝑖 = 𝒗 ⋅ 𝒏𝑖,
𝑖 = 1, 2, 3. 
where 𝒗 is a vector and {𝒏𝑖} are unit vectors aligned, respectively, 
with  the  global  axes  𝑥,  𝑦,  and  𝑧  axes.    Note  that  the  vector  𝒗  is 
attached to the body in question, so changing the direction of this
vector will induce a rotation of the body defined by 𝝋̇ = 𝒗 × 𝒗̇. 
LCIDS 
Load  curve  ID  which  specifies  the  overlayed  spin  speed    𝜃̇  of 
PIDB about the axis parallel to the vector 𝒗. 
EQ.0: a constant spin speed as defined by VALSPIN is used, 
GT.0:  Load curve for spin speed (radians per unit time). 
VALSPIN 
Value for the constant spin speed of PIDB (radians per unit time
𝜃̇).    This  option  is  bypassed  if  the  load  curve  number  defined
above is non-zero. 
𝜃̇
𝑛 
𝒗𝑛 
Time 𝑡𝑛 
𝜃̇
𝑛+1 
𝒗𝑛+1 
Time 𝑡𝑛+1
Total spin 𝝎 given by 
𝝎 = 𝝋̇ + 𝜽̇ = 𝒗 × 𝒗̇ + 𝜃̇𝒗 
Remarks: 
1.  All load curves must contain the same number of points and the data must be 
uniformly spaced. 
2.  LC0  in  *MAT_RIGID  must  be  used  to  identify  a  coordinate  system  for  each 
rigid  body.    The  coordinate  system  must  be  defined  with  *DEFINE_COORDI-
NATE_NODES  and  FLAG = 1.    Nodes  used  in  defining  the  coordinate  system 
must reside on the same body. 
3.  This feature is incompatible with *DEFINE_CURVE_FUNCTION.
*BOUNDARY_PRESSURE_OUTFLOW_OPTION 
Available options include: 
SEGMENT 
SET 
Purpose:    Define  pressure  outflow  boundary  conditions.    These  boundary  conditions 
are  attached  to  solid  elements  using  the  Eulerian  ambient  formulation  (refer  to 
ELFORM  in  *SECTION_SOLID_ALE)  and  defined  to  be  pressure  outflow  ambient 
elements (refer to AET in *SECTION_SOLID_ALE). 
Card 1 for SET option. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
Type 
I 
Default 
none 
Card 1 for SEGMENT option. 
  Card 1 
Variable 
1 
N1 
Type 
I 
2 
N2 
I 
3 
N3 
I 
4 
N4 
I 
Default 
none 
none 
none 
none 
5 
6 
7 
8 
  VARIABLE   
DESCRIPTION
SSID 
Segment set ID 
N1, N2, … 
Node ID’s defining segment
*BOUNDARY_PWP_OPTION 
Available options include: 
NODE 
SET 
TABLE 
TABLE_SET 
Purpose:  Define pressure boundary conditions for pore water, e.g.  at soil surface.  The 
TABLE option applies to a whole Part, while the other options apply to specified nodes. 
  Card 1 
1 
Variable 
typeID 
Type 
I 
2 
LC 
F 
3 
4 
5 
6 
7 
8 
CMULT 
LCDR 
TBIRTH 
TDEATH 
F 
I 
F 
F 
Default 
none 
none 
0.0 
none 
0.0 
1020 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IPHRE 
ITOTEX 
IDRFLAG 
TABLE 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
typeID 
LC 
Node ID (option = NODE) or Node set ID (option = SET) or Part 
ID (option = TABLE) or Part Set ID (option = TABLE_SET) 
Load  curve  or  function  giving  pore  water  pressure  head  (length
units) vs time. 
EQ.0: constant pressure head assumed equal to CMULT 
(leave blank for TABLE option)
VARIABLE   
DESCRIPTION
CMULT 
Factor on curve or constant pressure head if LC = 0 
LCDR 
Load  curve  or  function  giving  pore  water  pressure  head  during
dynamic relaxation. 
EQ.0: during dynamic relaxation, use first pressure head value
on LC 
(leave blank for TABLE option) 
TBIRTH 
Time at which boundary condition becomes active 
TDEATH 
Time at which boundary condition becomes inactive 
IPHRE 
EQ.0: default behavior 
EQ.1: for  phreatic  behavior  (water  can  be  removed  by  the
boundary condition but not added, e.g.  at a sloping free 
surface).  Not applicable to TABLE option.  See remarks. 
ITOTEX 
Flag for type of pressure boundary condition:  
EQ.0: Total head 
EQ.1: Excess head 
EQ.2: Hydraulic head 
EQ.4: 𝑧-coord where head = 0 (piezometric level) 
IDRFLAG 
Active flag: 
EQ.0: Active only in transient analysis 
EQ.1: Active only in dynamic relaxation 
EQ.2: Active in all analysis phases 
(leave blank for TABLE option) 
TABLE 
Table ID for TABLE option only.  See notes below. 
Remarks: 
1.  Pressure is given as pressure head, i.e.  pressure/ρg. 
2.  NODE  and  SET  options  do  not  affect  the  pore  pressure  in  Drained  parts  (the 
pore pressure for these is set on a part basis and overrides any nodal boundary 
conditions).  The TABLE option should be used only with Drained parts.
3. 
4. 
*BOUNDARY_PWP_NODE  or  SET  overrides  pressure  head  from  *BOUND-
ARY_PWP_TABLE at nodes where both are present.  
4.  If LC is a *DEFINE_FUNCTION, the input arguments are (time, x, y, z, x0, 
y0, z0) where x, y and z are the current coordinates and x0, y0, z0 are the initial 
coordinates of the node. 
TABLE and TABLE_SET options: 
The table consists of a list of times in ascending order, followed immediately by curves 
of  𝑧-coordinate  versus  pore  pressure  head.    Each  curve  represents  the  pore  water 
pressure head distribution with 𝑧-coordinate at the corresponding time.  There must be 
the same number of curves as time values, arranged immediately after the *DEFINE_-
TABLE and in the correct order to correspond to the time values.  Each curve should be 
arranged in ascending order of 𝑧-coordinate – they look upside-down on the page.  The 
𝑧-coordinate is the 𝑥-axis of the curve, the pore water pressure head (in length units) is 
the y-axis.  Each curve should have the same 𝑧-coordinates (𝑥-values) and use the same 
value of LCINT.  Ensure that the range of 𝑧-coordinates in the curve exceeds by at least 
5% the range of 𝑧-coordinates of the nodes belonging to the parts to which the boundary 
condition is applied. 
IPHRE: 
“Phreatic” means that water can be removed by the boundary condition but not added.  
The  boundary  condition  enforces  that  the  pressure  head  be  less  than  or  equal  to  the 
stated value.  This condition occurs when the free surface of the soil is sloping so that 
any water emerging from the soil runs away down the slope. 
ITOTEX = 0: 
The value from curve or table is total head.  This may be used with any pore pressure 
analysis type. 
ITOTEX = 1: 
The value from curve or table is excess head.  Total head will be determined by adding 
the  hydrostatic  head.    This  option  cannot  be  used  with  drained  analysis,  which  sets 
excess head to zero. 
ITOTEX = 2: 
The  value  from  curve  or  table  is  hydraulic  head,  to  which  excess  head  may  be  added 
due to volume change in the soil if the analysis type is not drained.
*BOUNDARY 
The curve value is the z-coordinate of the water surface; pore pressure head at any node 
in this boundary condition is given by, 
𝑧surface − 𝑧node 
This  option  allows  a  single  boundary  condition  to  be  used  for  nodes  at  any  depth, 
provided  that  the  pressure  distribution  is  hydrostatic  below  the  given  surface.    This 
option is not available for the TABLE option.
*BOUNDARY_RADIATION_OPTION1_{OPTION2}_{OPTION3} 
Available values for OPTION1 include: 
SET 
SEGMENT 
Available values for OPTION2 include: 
VF_READ 
VF_CALCULATE 
<BLANK> 
Available values for OPTION3 include: 
RESTART 
<BLANK> 
OPTION1 specifies radiation boundary surface definition by a surface set (SET) or by a 
segment list (SEGMENT).  
OPTION2 indicates the radiation boundary surface is part of an enclosure.  When set to 
VF  OPTION2  specifies  the  use  of  view  factors.    The  suffix,  READ,  indicates  that  the 
view factors should be read from the file “viewfl”.  The suffix, CALCULATE, indicates 
that  the  view  factors  should  be  calculated.    The  Stefan  Boltzmann  constant  must  be 
defined  for  radiation  in  an  enclosure  on  the  *CONTROL_THERMAL_SOLVER 
keyword.    The  parameter  DTVF  entered  on  the  CONTROL_THERMAL_SOLVER 
keyword defines the time interval between VF updates for moving geometries. 
OPTION3 is the keyword suffix RESTART.  This is only applicable in combination with 
the  keyword  VF_CALCULATE.    In  very  long  runs,  it  may  be  necessary  to  halt 
execution.    This  is  accomplished  by  entering  Ctrl-C  followed  by  sw1.    To  restart  the 
view  factor  calculation,  add  the  suffix  RESTART  to  all  VF_CALCULATE  keywords  in 
the input file. 
The  status  of  an  in-progress  view  factor  calculation  can  be  determined  by  using  the 
sense switch.  This is accomplished by first typing Control-C followed by: 
sw1. 
sw2. 
Stop run and save viewfl file for restart 
Viewfactor run statistics 
A list of acceptable keywords are: 
*BOUNDARY_RADIATION_SEGMENT
*BOUNDARY_RADIATION_SEGMENT_VF_READ 
*BOUNDARY_RADIATION_SEGMENT_VF_CALCULATE 
*BOUNDARY_RADIATION_SET 
*BOUNDARY_RADIATION_SET_VF_READ 
*BOUNDARY_RADIATION_SET_VF_CALCULATE 
Remarks: 
In  models  that  include  radiation  boundary  conditions,  a  thermodynamic  temperature 
scale  is  required,  i.e.,  zero  degrees  must  correspond  to  absolute  zero.    The  Kelvin  and 
Rankine  temperature  scales  meet  this  requirement  whereas  Celsius  and  Fahrenheit 
temperature scales do not.
*BOUNDARY_RADIATION_SEGMENT 
Include the following 2 cards for each segment.  Apply a radiation boundary condition 
on  a  SEGMENT  to  transfer  heat  between  the  segment  and  the  environment.    Setting 
TYPE = 1 on Card 1 below indicates that the segment transfers heat to the environment. 
  Card 1 
Variable 
1 
N1 
Type 
I 
2 
N2 
I 
3 
N3 
I 
4 
N4 
I 
Default 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
TYPE 
I 
1 
5 
6 
7 
8 
Variable 
FLCID 
FMULT 
TLCID 
TMULT 
LOC 
Type 
I 
F 
I 
F 
Default 
none 
0. 
none 
0. 
I 
0 
  VARIABLE   
DESCRIPTION
N1, N2, 
N3, N4 
TYPE 
FLCID 
Node ID’s defining segment 
Radiation type: 
EQ.1: Radiation to environment 
Radiation  heat  transfer  coefficient,  𝑓 = 𝜎𝜀𝐹,  specification  where 
σ = Stefan Boltzmann constant, ε = surface emissivity, F = surface 
view  factor.    This  parameter  can  reference  a  load  curve  ID    or  a  function  ID  .  When the reference is to a curve, FLCID has the 
following interpretation: 
GT.0:  𝑓   is  defined  as  a  function  of  time,  𝑡,  having  points 
consisting of (𝑡, 𝑓 (𝑡)) data pairs. 
EQ.0: 𝑓  is a constant defined by the value FMULT.
VARIABLE   
DESCRIPTION
LT.0:  𝑓   is  defined  as  a  function  of  temperature,  𝑇,  by  a  curve 
consisting of (𝑇, 𝑓 (𝑇) ) data pairs.  Enter |FLCID| on the 
DEFINE_CURVE keyword. 
FMULT 
Radiation  heat  transfer  coefficient,  f,  curve  multiplier  for  use  in
the equation 
q̇′′ = 𝜎𝜀𝐹(𝑇surface
− 𝑇∞
4 ) = 𝑓 (𝑇surface
− 𝑇∞
4 ) 
TLCID 
If  f  is  a  function  of  temperature,  f  is  evaluated  at  the  surface 
temperature, Tsurface.  [σ = Stefan Boltzmann constant, ε = surface 
emissivity, F = surface view factor] 
Environment temperature, 𝑇∞,  specification.    This  parameter  can 
reference a load curve ID  or a function ID 
.  When the reference is 
to a curve, TLCID has the following interpretation: 
GT.0:  𝑇∞  is  defined  as  a  function  of  time,  𝑡,  by  a  curve 
consisting of (𝑡, 𝑇∞(𝑡) ) data pairs. 
EQ.0: 𝑇∞ a constant defined by the value TMULT. 
TMULT 
Environment temperature, 𝑇∞, curve multiplier. 
LOC 
For  a  thick  thermal  shell,  the  radiation  will  be  applied  to  the
surface  identified  by  LOC.    See  the  parameter  THSHEL  on  the
*CONTROL_SHELL keyword. 
EQ.-1:  lower surface of thermal shell element 
EQ.0:  middle surface of thermal shell element 
EQ.1:  upper surface of thermal shell element 
Remarks: 
A radiation boundary condition is calculated using 
q̇′′ = 𝜎𝜀𝐹(𝑇surface
− 𝑇∞
4 ) = 𝑓 (𝑇surface
− 𝑇∞
4 ) 
Where, 𝑓   , is the radiation heat transfer coefficient.  If 𝑓  is a function of temperature, 𝑓 ,  
is evaluated at the surface temperature, Tsurface.  
1. 
If HLCID references a DEFINE_FUNCTION, the following function arguments 
are allowed 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑇, 𝑇∞, 𝑡) where: 
𝑥, 𝑦, 𝑧 = segment centroid coordinates
𝑣𝑥, 𝑣𝑦, 𝑣𝑧 = segment centroid velocity component 
T = segment centroid temperature 
𝑇∞ = environment temperature, T∞ 
𝑡 = solution time 
2. 
If TLCID references a DEFINE_FUNCTION, the following function arguments 
are allowed 𝑓 ( 𝑥 , 𝑦 , 𝑧 , 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡) where: 
𝑥, 𝑦, 𝑧 = segment centroid coordinates 
𝑣𝑥, 𝑣𝑦, 𝑣𝑧 = segment centroid velocity components 
𝑡 = solution time
*BOUNDARY_RADIATION_SEGMENT_VF_OPTION 
Available options include: 
READ 
CALCULATE 
Include the following 2 cards for each segment.  Apply a radiation boundary condition 
on a SEGMENT to transfer heat between the segment and an enclosure surrounding the 
segment using view factors.  The enclosure is defined by additional segments using this 
keyword.    Setting  TYPE = 2  on  Card  1  below  specifies  that  the  segment  belongs  to  an 
enclosure. 
The file “viewfl” must be present for the READ option, whereas it will be created with 
the  CALCULATE  option.    If  the  file  “viewfl”  exists  when  using  the  CALCULATE 
option, LS-DYNA will terminate with an error message to prevent overwriting the file.  
The file “viewfl” contains the surface-to-surface area × view factor products (i.e., 𝐴𝑖𝐹𝑖𝑗).  
These products are stored by row and formatted as 5E16.0. 
  Card 1 
Variable 
1 
N1 
Type 
I 
2 
N2 
I 
3 
N3 
I 
4 
N4 
I 
Default 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
TYPE 
BLOCK 
NINT 
I 
2 
5 
I 
0 
6 
I 
0 
7 
8 
Variable 
SELCID 
SEMULT 
Type 
I 
F 
Default 
none 
0. 
  VARIABLE   
DESCRIPTION
N1, N2, 
N3, N4 
Node ID’s defining segment
VARIABLE   
DESCRIPTION
TYPE 
Radiation type: 
EQ.2: Radiation within an enclosure 
BLOCK 
Flag indicating if this surface blocks the view between any other 2 
surfaces. 
EQ.0: no blocking (default) 
EQ.1: blocking 
NINT 
Number of integration points for viewfactor calculation 
EQ.0: 
LS-DYNA determines the number of integration 
points based on the segment size and separation 
distance 
1 ≤ NINT ≤ 10: User specified number 
SELCID 
Load curve ID for surface emissivity, see *DEFINE_CURVE 
GT.0:  function versus time 
EQ.0: use constant multiplier value, SEMULT 
LT.0:  function  versus  temperature.    The  value  of  –SELCID 
must  be  an  integer,  and  it  is  interpreted  as  a  load  curve
ID.  See the DEFINE_CURVE keyword. 
SEMULT 
Curve multiplier for surface emissivity, see *DEFINE_CURVE
*BOUNDARY 
Include the following 2 cards for each set.  Apply a radiation boundary condition on a 
SEGMENT_SET to transfer heat between the segment set and the environment Setting 
TYPE = 1  on  Card  1  below  indicates  that  the  segment  transfers  energy  to  the 
environment. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
TYPE 
Type 
I 
Default 
none 
  Card 2 
1 
I 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FLCID 
FMULT 
TLCID 
TMULT 
LOC 
Type 
I 
F 
I 
F 
Default 
none 
0. 
none 
0. 
I 
0 
  VARIABLE   
SSID 
DESCRIPTION
SSID specifies the ID for a set of segments that comprise a portion
of, or possibly, the entire enclosure.  See *SET_SEGMENT. 
TYPE 
Radiation type: 
EQ.1: Radiation to environment 
FLCID 
Radiation  heat  transfer  coefficient,    𝑓 = 𝜎𝜀𝐹,  specification  where 
σ = Stefan Boltzmann constant, ε = surface emissivity, F = surface 
view  factor.    This  parameter  can  reference  a  load  curve  ID    or  a  function  ID  .  When the reference is to a curve, FLCID has the 
following interpretation: 
GT.0:  𝑓  is defined as a function time, 𝑡, by a curve consisting of 
(𝑡, 𝑓 (𝑡)) data pairs.
VARIABLE   
DESCRIPTION
EQ.0: 𝑓  is a constant defined by the value FMULT. 
LT.0:  𝑓   is  defined  as  a  function  of  temperature,  𝑇,  by  a  curve 
consisting  of  (𝑇, 𝑓 (𝑇))  data  pairs.    Enter  |-FLCID|  on 
the DEFINE_CURVE keyword 
FMULT 
Curve multiplier for f  for use in the equation 
q̇′′ = 𝜎𝜀𝐹(𝑇surface
− 𝑇∞
4 ) = 𝑓 (𝑇surface
− 𝑇∞
4 ) 
TLCID 
If  f  is  a  function  of  temperature,  f  is  evaluated  at  the  surface
temperature, Tsurface.  [σ = Stefan Boltzmann constant, ε = surface 
emissivity, F = surface view factor] 
Environment temperature, 𝑇∞ , specification.  This parameter can 
reference a load curve ID  or a function ID 
.  When the reference is 
to a curve, TLCID has the following interpretation: 
GT.0:  𝑇∞  is  defined  as  a  function  of  time,  𝑡,  by  a  curve 
consisting of (𝑡, 𝑇∞(𝑡)) data pairs. 
EQ.0: 𝑇∞ a constant defined by the value TMULT 
TMULT 
Curve multiplier for 𝑇∞ 
LOC 
For  a  thick  thermal  shell,  the  radiation  will  be  applied  to  the
surface  identified  by  LOC.    See  the  parameter  THSHEL  on  the
*CONTROL_SHELL keyword. 
EQ.-1:  lower surface of thermal shell element 
EQ.0.:  middle surface of thermal shell element 
EQ.1:  upper surface of thermal shell element 
Remarks: 
A radiation boundary condition is calculated using 
q̇′′ = 𝜎𝜀𝐹(𝑇surface
− 𝑇∞
4 ) = 𝑓 (𝑇surface
− 𝑇∞
4 ) 
Where,  f  , is the radiation heat transfer coefficient.  . If f is a function of temperature, f,  
is evaluated at the surface temperature, Tsurface.  
1. 
If HLCID references a DEFINE_FUNCTION, the following function arguments 
are allowed 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑇, 𝑇∞, 𝑡) where:
𝑥, 𝑦, 𝑧 = segment centroid coordinates 
𝑣𝑥, 𝑣𝑦, 𝑣𝑧 = segment centroid velocity component 
𝑇 = segment centroid temperature 
𝑇∞ = environment temperature, T∞ 
𝑡 = solution time 
2. 
If TLCID references a DEFINE_FUNCTION, the following function arguments 
are allowed 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡) where: 
𝑥, 𝑦, 𝑧 = segment centroid coordinates 
𝑣𝑥, 𝑣𝑦, 𝑣𝑧 = segment centroid velocity components 
𝑡 = solution time
*BOUNDARY_RADIATION_SET_VF_OPTION 
Available options include: 
READ 
CALCULATE 
Include the following 2 cards for each set.  Apply a radiation boundary condition on a 
SEGMENT_SET to transfer heat between the segment set and an enclosure surrounding 
the segments using view factors.  Segments contained in the SEGMENT_SET may form 
the enclosure.  Setting TYPE = 2 on Card 1 below specifies that the segment set belongs 
to an enclosure. 
The file “viewfl” must be present for the READ option.  The file “viewfl” will be created 
for  the  CALCULATE  option.    If  the  file  “viewfl”  exists  when  using  the  CACULATE 
option, LS-DYNA will terminate with an error message to prevent overwriting the file.  
The file “viewfl” contains the surface-to-surface area × view factor products (i.e. 𝐴𝑖𝐹𝑖𝑗).  
These products are stored by row and formatted as 5E16.0. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
TYPE 
RAD_GRP FILE_NO 
BLOCK 
NINT 
Type 
I 
Default 
none 
  Card 2 
1 
I 
2 
2 
I 
0 
3 
I 
0 
4 
I 
0 
5 
I 
0 
6 
7 
8 
Variable 
SELCID 
SEMULT 
Type 
I 
F 
Default 
none 
0. 
  VARIABLE   
SSID 
DESCRIPTION
SSID specifies the ID for a set of segments that comprise a portion
of, or possibly, the entire enclosure.  See *SET_SEGMENT.
VARIABLE   
DESCRIPTION
TYPE 
Radiation type: 
EQ.2: Radiation within an enclosure 
RAD_GRP 
FILE_NO 
Radiation  enclosure  group  ID.    The  segment  sets  from  all
radiation  enclosure  definitions  with  the  same  group  ID  are
augmented to form a single enclosure definition.  If RAD_GRP is 
not specified or set to zero, then the segments are placed in group
zero.    All  segments  defined  by  the  SEGMENT  option  are  placed 
in set zero. 
File  number  for  view factor file.    FILE_NO  is  added  to  “viewfl_”
to  form  the  name  of  the  file  containing  the  view  factors.    For
example  if  FILE_NO  is  specified  as  22,  then  the  view  factors  are
read  from  viewfl_22.    For  radiation  enclosure  group  zero  FILE_-
NO  is  ignored  and  view  factors  are  read  from  viewfl.    The  same 
file  may  be  used  for  different  radiation  enclosure  group
definitions. 
BLOCK 
Flag indicating if this surface blocks the view between any other 2
surfaces. 
EQ.0: no blocking (default) 
EQ.1: blocking 
NINT 
Number of integration points for viewfactor calculation 
EQ.0:  LS-DYNA  determines  the  number  of  integration  points
based on the segment size and separation distance 
GE.11: Not allowed 
SELCID 
Load curve ID for surface emissivity, see *DEFINE_CURVE 
GT.0: function versus time 
EQ.0: use constant multiplier value, SEMULT 
LT.0:  function  versus  temperature.    Enter  –SELCID  as  |-
SELCID| on the DEFINE_CURVE keyword. 
SEMULT 
Curve multiplier for surface emissivity, see *DEFINE_CURVE
*BOUNDARY_RADIATION_SET_VF 
Multiple enclosures can be modeled when using view factors.  Consider the following 
example input.  The order of segments in the view factor file follows the order the sets 
are assigned to the boundary radiation definition. 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *BOUNDARY_RADIATION_SET 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Make boundary enclosure radiation groups 8 and 9. 
$ 
*BOUNDARY_RADIATION_SET_VF_READ 
*      SSID      TYPE   RAD_GRP   FILE_NO 
        15         2         9        10 
       1.0       1.0 
*BOUNDARY_RADIATION_SET_VF_READ 
*      SSID      TYPE   RAD_GRP   FILE_NO 
        12         2         9        10 
       1.0       1.0 
*BOUNDARY_RADIATION_SET_VF_READ 
*      SSID      TYPE   RAD_GRP   FILE_NO 
        13         2         8        21 
       1.0       1.0 
$ 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
Enclosure radiation group 9 is composed of all the segments in segment set 15 followed 
by those in segment set 12.  The view factors are stored in the file viewfl_10.  Enclosure 
radiation group 8 is composed of the segments in segment set 13.  The view factors are 
stored in the file viewfl_21.
*BOUNDARY 
Purpose:  Define a sliding symmetry plane.  This option applies to continuum domains 
modeled with solid elements. 
  Card 1 
1 
Variable 
NSID 
Type 
I 
Default 
none 
2 
VX 
F 
0 
3 
VY 
F 
0 
4 
VZ 
F 
0 
5 
6 
7 
8 
COPT 
I 
0 
  VARIABLE   
DESCRIPTION
NSID 
Nodal set ID, see *SET_NODE 
VX 
VY 
VZ 
x-component of vector defining normal or vector 
y-component of vector defining normal or vector 
z-component of vector defining normal or vector 
COPT 
Option: 
EQ.0: node moves on normal plane, 
EQ.1: node moves only in vector direction. 
Remarks: 
Any  node  may  be  constrained  to  move  on  an  arbitrarily  oriented  plane  or  line 
depending  on  the  choice  of  COPT.    Each  boundary  condition  card  defines  a  vector 
originating  at  (0,  0,  0)  and  terminating  at  the  coordinates  defined  above.    Since  an 
arbitrary  magnitude  is  assumed  for  this  vector,  the  specified  coordinates  are  non-
unique  and  define  only  a  direction.    Use  of  *BOUNDARY_SPC  is  preferred  over 
*BOUNDARY_SLIDING_PLANE  as  the  boundary  conditions  imposed  via  the  latter 
have  been  seen  to  break  down  somewhat  in  lengthy  simulations  owing  to  numerical 
roundoff.
*BOUNDARY_SPC_OPTION1_{OPTION2}_{OPTION3} 
OPTION1 is required since it specifies whether the SPC applies to a single node or to a 
set.  The two choices are: 
NODE 
SET 
OPTION2 allows optional birth and death times to be assigned the single node or node 
set: 
BIRTH_DEATH 
This option requires one additional line of input.  The BIRTH_DEATH option is inactive 
during the dynamic relaxation phase, which allows the SPC to be removed during the 
subsequent normal analysis phase.  The BIRTH_DEATH option can be used only once 
for any given node and if used, no other *BOUNDARY_SPC commands can be used for 
that node. 
OPTION3 allows an optional ID to be given that applies either to the single node or to 
the entire set: 
ID 
If a heading is defined with the ID, then the ID with the heading will be written at the 
beginning of the ASCII file, spcforc. 
Purpose:    Define  nodal  single  point  constraints.    Do  not  use  this  option  in  r-adaptive 
problems  since  the  nodal  point  ID's  change  during  the  adaptive  step.    If  possible  use 
CONSTRAINED_GLOBAL instead. 
ID Card.  Additional card for the ID keyword option.  
 Optional 
Variable 
1 
ID 
Type 
I 
2 
3 
4 
5 
6 
7 
8 
HEADING 
A70
Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  NID/NSID 
CID 
DOFX 
DOFY 
DOFZ 
DOFRX 
DOFRY 
DOFRZ 
Type 
I 
Default 
none 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
Birth/Death Card.  Additional card for the BIRTH_DEATH keyword option.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BIRTH 
DEATH 
Type 
F 
F 
Default 
0.0 
1020 
  VARIABLE   
DESCRIPTION
ID 
Optional SPC set ID to which this node or node set belongs.  This
ID does not need to be unique 
HEADING 
An optional SPC descriptor that will be written into the d3hsp file 
and the spcforc file. 
NID/NSID 
Node ID or nodal set ID, see *SET_NODE. 
CID 
DOFX 
DOFY 
DOFZ 
Coordinate system ID, see *DEFINE_COORDINATE_SYSTEM. 
Insert 1 for translational constraint in local 𝑥-direction. 
Insert 1 for translational constraint in local 𝑦-direction. 
Insert 1 for translational constraint in local 𝑧-direction. 
DOFRX 
Insert 1 for rotational constraint about local 𝑥-axis. 
DOFRY 
Insert 1 for rotational constraint about local 𝑦-axis. 
DOFRZ 
Insert 1 for rotational constraint about local 𝑧-axis.
VARIABLE   
DESCRIPTION
Activation  time  for  SPC  constraint.    The  birth  time  is  ignored
during dynamic relaxation. 
Deactivation  time  for  the  SPC  constraint.    The  death  time  is 
ignored during dynamic relaxation. 
BIRTH 
DEATH 
Remarks: 
Constraints  are  applied  if  for  each  DOFij  field  set  to  1.    A  value  of  zero  means  no 
constraint.    No  attempt  should  be  made  to  apply  SPCs  to  nodes  belonging  to  rigid 
bodies . 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *BOUNDARY_SPC_NODE 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Make boundary constraints for nodes 6 and 542. 
$ 
*BOUNDARY_SPC_NODE 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      nid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         6         0         1         1         1         1         1         1 
       542         0         0         1         0         1         0         1 
$ 
$      Node 6 is fixed in all six degrees of freedom (no motion allowed). 
$       
$      Node 542 has a symmetry condition constraint in the x-z plane, 
$        no motion allowed for y translation, and x & z rotation. 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
*BOUNDARY_SPC_SYMMETRY_PLANE_{OPTION} 
This  keyword  is  developed  to  create  nodal  symmetric  constraints  by  defining  a 
symmetric plane. 
Available options include: 
<BLANK> 
SET 
The  option  SET  allows  for  symmetric  boundary  conditions  to  be  applied  on  tailor-
welded blanks (TWB).   
Card Sets.  For each symmetry plane input one pair of cards 1 and 2.  This input ends at 
the next keyword (“*”) card. 
  Card 1 
1 
2 
Variable 
IDSP 
PID/PSID 
Type 
I 
I 
3 
X 
F 
4 
Y 
F 
5 
Z 
F 
6 
VX 
F 
7 
VY 
F 
8 
VZ 
F 
Default 
none 
none 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TOL 
Type 
F 
Default 
0.0 
  VARIABLE   
DESCRIPTION
IDSP 
Identification number of the constraint.  Must be unique. 
PID/PSID 
A part ID of the deformable part (sheet metal blank, for example)
on which the constraints will be imposed.  When the option SET
is invoked, a part set ID can be input.
VX, VY, VZ
X, Y, Z
TOL
TOL
All nodes within +/- TOL of the plane defined 
by the point with coordinate (X, Y, Z) and the 
plane with normal vector (VX, VY, VZ) will be 
constrained symmetrically.
  Figure 5-5.  Define symmetry constraints using the variables in the keyword.
  VARIABLE   
DESCRIPTION
X, Y, Z 
Position coordinates on the symmetry plane. 
VX, VY, VZ 
Vector components of the symmetry plane normal. 
TOL 
A  distance  tolerance  value  within  which  the  nodes  on  the
deformable part will be constrained. 
Remarks: 
1.  Adaptive refined nodes generated along the symmetry plane during simulation 
are automatically included in the constraints. 
2.  Figure  5-5  shows  an  example  of  applying  symmetry  constraints  using  the 
variables in the keyword. 
3.  The  following  keyword  creates  symmetric  constraints  on  nodes  (from  PID  11) 
within distance of 0.1mm from the defined symmetry plane (with normal vec-
tors [1.0,1.0,1.0]) that goes through point coordinates (10.5, 40.0, 20.0): 
*BOUNDARY_SPC_SYMMETRY_PLANE 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$     IDSP       PID         X         Y         Z        VX        VY        VZ 
         1        11      10.5      40.0      20.0       1.0       1.0       1.0 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      TOL
4.  The  following  keywords  create  two  symmetric  constraints  on  nodes  from  part 
set  ID  99  (which  includes  part  IDs  13  and  14)  within  distance  of  0.1mm  from 
two  defined  symmetry  planes  (with  normal  vectors  [1.0,  0.0,  0.0]  and  [0.0,  1.0, 
0.0],  respectively)  that  all  go  through  point  coordinates  (-76.0,  35.6,  0.0).   Note 
the two point coordinates that define the two symmetry planes must be exactly 
the same. 
*SET_PART_LIST 
99 
13,14 
*BOUNDARY_SPC_SYMMETRY_PLANE_SET 
$     IDSP       PID         X         Y         Z        VX        VY        VZ 
         1        99     -76.0      35.6       0.0       1.0 
$      TOL 
      0.10 
         2        99     -76.0      35.6       0.0       0.0       1.0 
$      TOL 
      0.10 
Revision information: 
This feature is available starting in Revision 85404.  The option SET is available starting 
in Revision 113355.
*BOUNDARY_SPH_FLOW 
Purpose:    Define  a  flow  of  particles.    This  option  applies  to  continuum  domains 
modeled with SPH elements. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
STYP 
DOF 
VAD 
LCID 
6 
SF 
F 
7 
8 
DEATH 
BIRTH 
F 
F 
I 
none 
1. 
1.E+20 
0.0 
5 
6 
7 
8 
I 
0 
4 
Type 
I 
I 
I 
Default 
none 
none 
none 
  Card 2 
1 
2 
3 
Variable 
NODE 
VID 
Type 
I 
Default 
none 
I 
0 
  VARIABLE   
NSID, PID 
DESCRIPTION
Nodal  set  ID  (NSID),  SEE  *SET_NODE,  or  part  ID  (PID),  see 
*PART. 
STYP 
Set type: 
EQ.1: part set ID, see *SET_PART, 
EQ.2: part ID, see *PART, 
EQ.3: node set ID, see *NODE_SET,
Node
boundary
vector VID
deactivated particle
activated particle
SPH Flow
Figure 5-6.  Vector VID determines the orientation of the SPH flow 
  VARIABLE   
DESCRIPTION
DOF 
Applicable degrees-of-freedom: 
EQ.1: x-translational degree-of-freedom, 
EQ.2: y-translational degree-of-freedom, 
EQ.3: z-translational degree-of-freedom, 
EQ.4: translational motion in direction given by the VID.  
Movement  on  plane  normal  to  the  vector  is  permitted.
VAD 
Velocity/Acceleration/Displacement 
elements before activation: 
flag  applied 
to  SPH
EQ.0: velocity, 
EQ.1: acceleration, 
EQ.2: displacement. 
LCID 
Load  curve  ID  to  describe  motion  value  versus  time,  see  *DE-
FINE_CURVE. 
SF 
Load curve scale factor.  (default = 1.0) 
DEATH 
Time imposed motion/constraint is removed: 
EQ.0.0: default set to 1020. 
BIRTH 
Time imposed motion/constraint is activated.
VARIABLE   
NODE 
DESCRIPTION
Node  fixed  in  space  which  determines  the  boundary  between 
activated particles and deactivated particles. 
VID 
Vector ID for DOF value of 4, see *DEFINE_VECTOR 
Remarks: 
Initially,  the  user  defines  the  set of  particles  that  are  representing the  flow  of  particles 
during the simulation.  At time t = 0, all the particles are deactivated which means that 
no  particle  approximation  is  calculated.    The  boundary  of  activation  is  a  plane 
determined  by  the  NODE,  and  normal  to  the  vector  VID.    The  particles  are  activated 
when  they  reached  the  boundary.    Since  they  are  activated,  particle  approximation  is 
started.
*BOUNDARY_SPH_NON_REFLECTING 
Purpose:    Define  a  non-reflecting  boundary  plane  for  SPH.    This  option  applies  to 
continuum domains modeled with SPH elements. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VTX 
VTY 
VTZ 
VHX 
VHY 
VHZ 
Type 
F 
Default 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
  VARIABLE   
DESCRIPTION
x-coordinate  of  tail  of  a  normal  vector  originating  on  the  wall
(tail) and terminating in the body (head) (i.e., vector points from
the non-reflecting boundary plane into the body). 
y-coordinate of tail 
z-coordinate of tail 
x-coordinate of head 
y-coordinate of head 
z-coordinate of head 
VTX 
VTY 
VTZ 
VHX 
VHY 
VHZ 
Remarks: 
1.  The  non-reflecting  boundary  plane  has  to  be  normal  to  either  the  x,  y  or  z 
direction.
*BOUNDARY_SPH_SYMMETRY_PLANE 
Purpose:  Define a symmetry plane for SPH.  This option applies to continuum domains 
modeled with SPH elements. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VTX 
VTY 
VTZ 
VHX 
VHY 
VHZ 
Type 
F 
Default 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
  VARIABLE   
DESCRIPTION
x-coordinate  of  tail  of  a  normal  vector  originating  on  the  wall
(tail) and terminating in the body (head) (i.e., vector points from
the symmetry plane into the body). 
y-coordinate of tail 
z-coordinate of tail 
x-coordinate of head 
y-coordinate of head 
z-coordinate of head 
VTX 
VTY 
VTZ 
VHX 
VHY 
VHZ 
Remarks: 
1.  A plane of symmetry is assumed for all SPH elements defined in the model. 
2.  The plane of symmetry has to be normal to either the x, y or z direction. 
3.  For axi-symmetric SPH analysis, IDIM = -2, a plane of symmetry centered at the 
global origin and normal to x-direction is automatically created by LS-Dyna.
*BOUNDARY_SYMMETRY_FAILURE 
Purpose:    Define  a  symmetry  plane  with  a  failure  criterion.    This  option  applies  to 
continuum domains modeled with solid elements. 
  Card 1 
1 
Variable 
SSID 
Type 
I 
2 
FS 
F 
Default 
none 
0. 
3 
4 
5 
6 
7 
8 
VTX 
VTY 
VTZ 
VHX 
VHY 
VHZ 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
  VARIABLE   
DESCRIPTION
Segment set ID, see *SET_SEGMENT 
Tensile  failure  stress > 0.0.    The  average  stress  in  the  elements 
surrounding  the  boundary  nodes  in  a  direction  perpendicular  to
the boundary is used. 
x-coordinate  of  tail  of  a  normal  vector  originating  on  the  wall 
(tail) and terminating in the body (head) (i.e., vector points from
the symmetry plane into the body). 
y-coordinate of tail 
z-coordinate of tail 
x-coordinate of head 
y-coordinate of head 
z-coordinate of head 
SSID 
FS 
VTX 
VTY 
VTZ 
VHX 
VHY 
VHZ 
Remarks: 
A plane of symmetry is assumed for the nodes on the boundary at the tail of the vector 
given  above.    Only  the  motion  perpendicular  to  the  symmetry  plane  is  constrained.  
After failure the nodes are set free.
*BOUNDARY_TEMPERATURE_OPTION 
Available options include: 
NODE 
SET 
Purpose:    Define  temperature  boundary  conditions  for  a  thermal  or  coupled  thermal/
structural analysis. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID/SID 
TLCID 
TMULT 
LOC 
Type 
I 
Default 
none 
I 
0 
F 
0. 
I 
0 
  VARIABLE   
DESCRIPTION
NID/SID 
Node ID/Node Set ID, see *SET_NODE_OPTION 
TLCID 
Temperature,  𝑇,  specification.    This  parameter  can  reference  a
load  curve  ID    or  a  function  ID  .    When  the  reference  is  to  a
curve, TLCID has the following interpretation: 
GT.0:  𝑇 is defined by a curve consisting of (𝑡, 𝑇) data pairs. 
EQ.0: 𝑇 is a constant defined by the value TMULT. 
TMULT 
Temperature, 𝑇, curve multiplier. 
LOC 
Application  of  surface  for  thermal  shell  elements,  see  parameter, 
THSHEL, in the *CONTROL_SHELL input: 
EQ.-1: lower surface of thermal shell element 
EQ.0:  middle surface of thermal shell element 
EQ.1:  upper surface of thermal shell element
Remarks: 
1.  This  keyword  can  be  used  to  apply  temperature  boundary  conditions  to  SPH 
particles. 
2. 
If TLCID references a DEFINE_FUNCTION, the following function arguments 
are allowed 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡): 
𝑥, 𝑦, 𝑧 = node point coordinates 
𝑣𝑥, 𝑣𝑦, 𝑣𝑧 = node point velocity components 
𝑡 = solution time
*BOUNDARY_THERMAL_BULKFLOW_OPTION1_OPTION2 
Purpose:  Used to define bulk fluid flow elements. 
OPTION1 is required since it specifies  whether the BULKFLOW applies to an element 
or set. 
ELEMENT 
SET 
OPTION2 if used turns on the fluid upwind algorithm 
UPWIND 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EID/SID 
LCID 
MDOT 
Type 
I 
I 
F 
Default 
none 
none 
none 
  VARIABLE   
EID / SID 
DESCRIPTION
Beam element ID (EID) for ELEMENT option 
Beam set ID (SID) for SET option 
LCID 
Load Curve ID for mass flow rate versus time. 
MDOT 
Mass flow rate (e.g.  kg/sec).
*BOUNDARY_THERMAL_BULKNODE 
Purpose:  Used to define thermal bulk nodes. 
  Card 1 
1 
2 
3 
4 
5 
Variable 
NID 
PID 
NBNSEG 
VOL 
LCID 
Type 
I 
I 
Default 
none 
none 
I 
0 
F 
none 
I 
0 
6 
H 
F 
0. 
7 
8 
AEXP 
BEXP 
F 
0. 
F 
0. 
Bulk Node Cards.  Include NBNSEG cards, one for each bulk node segment. 
  Card 2 
Variable 
1 
N1 
Type 
I 
2 
N2 
I 
3 
N3 
I 
4 
N4 
I 
5 
6 
7 
8 
  VARIABLE   
DESCRIPTION
NID 
PID 
VOL 
Bulk node number. 
Bulk node part ID. 
Bulk node volume. 
NBNSEG 
Number  of  element  surface  segments  that  transfer  heat  with
this bulk node. 
N1, N2, N3, N4 
Nodal point numbers 
LCID 
H 
AEXP 
BEXP 
Load curve ID for H 
Heat transfer coefficient 
𝑎 exponent 
𝑏 exponent
*BOUNDARY_THERMAL_BULKNODE 
The heat flow between a bulk node (TB) and a bulk node segment (TS) is given by 
𝑞 = ℎ(𝑇𝐵
𝑎 − 𝑇𝐵
𝑎 )𝑏 
1.  For convection, set 𝑎 = 𝑏 = 1. 
2.  For radiation, set 𝑎 = 4, 𝑏 = 1. 
3.  For  flux,  set 𝑎 = 𝑏 = 0.    Mathematically,  anything  to  the  0  power  is  1.    This 
= (1 − 1)0 = 00 = 1.    However,  some  com-
to  set 
It 
produces  the  expression, (𝑇𝐵
puter  operating  systems  don’t 
𝑎 = 𝑏 = very small number.
recognize  00. 
0)
0−𝑇𝑆
is  safer
*BOUNDARY_THERMAL_WELD 
Purpose:  Define a moving heat source to model welding.  Only applicable for a coupled 
thermal-structural simulations in which the weld source or work piece is moving. 
  Card 1 
1 
2 
3 
4 
Variable 
PID 
PTYP 
NID 
NFLAG 
Type 
I 
Default 
none 
  Card 2 
Variable 
Type 
1 
a 
F 
I 
1 
2 
b 
F 
I 
none 
3 
cf 
F 
I 
1 
4 
cr 
F 
5 
X0 
F 
6 
Y0 
F 
7 
Z0 
F 
8 
N2ID 
I 
none 
none 
none 
none 
5 
LCID 
I 
6 
Q 
F 
7 
Ff 
F 
8 
Fr 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Beam Aiming Direction Card.   Additional card for N2ID = -1. 
4 
5 
6 
7 
8 
 Optional 
Variable 
1 
TX 
Type 
F 
2 
TY 
F 
3 
TZ 
F 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION
PID 
PTYP 
Part ID or Part Set ID to which weld source is applied 
PID type: 
EQ.1: PID defines a single part ID 
EQ.2: PID defines a part set ID
Welding
Torch
velocity
cr
cf
(a)
(b)
Figure  5-7.    Schematic  illustration  of  welding  with  moving  torch.    The  left
figure (a) shows the surface of the material from above, while the right figure
(b) shows a slice along the dotted line in the y-z plane. 
  VARIABLE   
DESCRIPTION
NID 
Node ID giving location of weld source 
EQ.0: location defined by (X0, Y0, Z0) below 
NFLAG 
Flag controlling motion of weld source 
EQ.1: source moves with node NID 
EQ.2: source is fixed in space at original position of node NID 
X0, Y0, Z0 
Coordinates  of  weld  source,  which  remains  fixed  in  space
(optional, ignored if NID nonzero above) 
N2ID 
Second node ID for weld beam aiming direction 
GT.0:  beam  is  aimed  from  N2ID  to  NID,  moves  with  these
nodes 
EQ.-1: beam  aiming  direction  is  (tx,  ty,  tz)  input  on  optional 
card 3 
a 
b 
cf 
cr 
Weld pool radius (i.e., half width) 
Weld pool depth (in beam aiming direction) 
Weld pool forward direction 
Weld pool rearward direction
VARIABLE   
DESCRIPTION
LCID 
Load curve ID for weld energy input rate vs.  time 
EQ.0: use constant multiplier value Q. 
Q 
Ff 
Fr 
Curve  multiplier  for  weld  energy  input  rate  [energy/time,  e.g.,
Watt]  
LT.0:  use absolute value and accurate integration of heat 
Forward distribution function 
Rear distribution function (Note:Ff + Fr = 2.0) 
TX, TY, TZ 
Weld  beam  direction  vector  in  global  coordinates    (N2ID = -1 
only) 
Remarks:  
This boundary condition allows simulation of a moving weld heat source, following the 
work  of  Goldak,  Chakravarti,  and  Bibby  [1984].    Heat  is  generated  in  an  ellipsoidal 
region centered at the weld source, and decaying exponentially with distance according 
to: 
where: 
𝑞 =
6√3𝐹𝑄
𝜋√𝜋𝑎𝑏𝑐
exp (
−3𝑥2
𝑎2 ) exp (
−3𝑦2
𝑏2 ) exp (
−3𝑧2
𝑐2 ) 
𝑞 = weld source power density 
(𝑥, 𝑦, 𝑧) = coordinates of point 𝑝 in weld material 
𝐹 = {
𝑐 = {
Ff if point 𝑝 is in front of beam
Fr if point 𝑝 is behind beam
cf if point 𝑝 is in front of beam
cr if point 𝑝 is behind beam
A  local  coordinate  system  is  constructed  which  is  centered  at  the  heat  source.    The 
relative  velocity  vector  of  the  heat  source  defines  the  "forward"  direction,  so  material 
points that are approaching the heat source are in "front" of the beam.  The beam aiming 
direction  is  used  to  compute  the  weld  pool  depth.    The  weld  pool  width  is  measured 
normal to the relative velocity - aiming direction plane.  If Q is defined negative in the 
input,  then  the  formula  above  is  using  the  absolute  value  of  Q,  and  a  more  accurate 
integration of the heat source is performed with some additional cost in CPU time. 
To  simulate  a  welding  process  during  which  the  welding  torch  is  fixed  in  space,  NID 
and  N2ID  must  be  set  to  0  and  -1  respectively.    The  X0,  Y0,  and  Z0  fields  specify  the
global  coordinates  of  the  welding  torch,  and  the  TX,  TY,  and  TZ  fields  specify  the 
direction  of  the  welding  beam.    The  motion  of  the  work  piece  is  prescribed  using  the 
*BOUNDARY_PRESCRIBED_MOTION keyword. 
To simulate a welding process for which the work piece fixed in space, NID and N2ID 
specify  both  the  beam  source  location  and  direction.    The  X0,  Y0,  Z0,  TX,  TY,  and  TZ 
fields are ignored.  The motion of welding source is prescribed with using the *BOUND-
ARY_PRESCRIBED_MOTION keyword applied to the two nodal points specified in the 
NID and N2ID fields.
*BOUNDARY_THERMAL_WELD_TRAJECTORY 
Purpose:    Define  a  moving  heat  source  to  model  welding  of  solid  or  shell  structures.  
Motion of the source is described by a nodal path and a prescribed velocity on this path.  
This keyword is applicable in coupled thermal-structural and thermal-only simulations 
and also supports thermal dumping.  Different equivalent heat source descriptions are 
implemented. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
PTYP 
NSID1 
VEL1 
SID2 
VEL2 
NCYC 
RELVEL 
Type 
I 
Default 
none 
  Card 2 
1 
I 
1 
2 
Variable 
IFORM 
LCID 
Type 
I 
I 
I 
F 
I 
F 
none 
none 
none 
none 
3 
Q 
F 
4 
5 
6 
LCROT 
LCMOV 
LCLAT 
DISC 
I 
I 
I 
F 
I 
1 
7 
Default 
none 
none 
none 
none 
none 
none 
none 
  Card 3 
Variable 
1 
P1 
Type 
F 
2 
P2 
F 
3 
P3 
F 
4 
P4 
F 
5 
P5 
F 
6 
P6 
F 
7 
P7 
F 
I 
0 
8 
8 
P8 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none
Weld Source Aiming Direction Card.   Additional card for NS2ID = 0. 
4 
5 
6 
7 
8 
 Optional 
Variable 
1 
TX 
Type 
F 
2 
TY 
F 
3 
TZ 
F 
Default 
none 
none 
none 
  VARIABLE   
PID 
DESCRIPTION
Part ID or Part Set ID of solids or shells to which  weld  source is 
applied 
PTYP 
PID type: 
EQ.1: PID defines a single part ID 
EQ.2: PID defines a part set ID 
NSID1 
Node set ID containing the path (weld trajectory) information for
the weld source movement.  A sorted node set is requested.  The
order defines the weld path and the direction .  
VEL1 
Velocity of the heat source on the weld trajectory 
GT.0: constant velocity 
LT.0:  |VEL1| is a load curve ID defining weld speed vs.  time 
SID2 
ID  of  second  node  set  or  segment  set  containing  information  for 
the weld source aiming direction  
GT.0:  SID2  refers  to  a  sorted  node  set,  the  order  of  which
defines the direction of the trajectory.  The heat source is
aimed from current position in SID2 to current position
in the weld trajectory.  
EQ.0:  beam aiming direction is (tx, ty, tz) input on optional 
card 4. 
LT.0:   |SID2| is a segment set.  The heat source is aiming in 
normal direction to segments in the set.
VARIABLE   
DESCRIPTION
VEL2 
Velocity of reference point in SID2, if SID2 > 0 
GT.0: constant velocity 
LT.0:  |VEL2| is a load curve ID defining weld speed vs.  time 
NCYC 
RELVEL 
Number  of  substeps  for  subcycling  in  evaluation  of  boundary
condition.  Allows thermal dumping . 
Defines  if  VEL1  and  VEL2  are  relative  or  absolute  velocities  in 
coupled simulations  
EQ.0: absolute velocities 
EQ.1: relative velocities with respect to underlying structure 
IFORM 
Geometry  description  for  energy  rate  density  distribution  : 
EQ.1: Goldak-type heat source 
EQ.2: double ellipsoidal heat source with constant density 
EQ.3: double conical heat source with constant density 
EQ.4: frustum-shaped heat source with constant density 
LCID 
Load curve ID for weld energy input rate vs.  time 
EQ.0: use constant multiplier value Q. 
Q 
Curve multiplier for weld energy input rate [energy/time]  
LT.0:  take absolute value and accurate integration of heat using
integration cells with edge length DISC. 
LCROT 
LCMOV 
LCLAT 
DISC 
Load curve defining the rotation (angle in degree) of weld source 
around the trajectory as function of time . 
Load curve for offset of weld source in direction of the weld beam
as function of time  
Load  curve  for  lateral  offset  of  weld  source  as  function  of  time
 
Resolution  for  accurate  integration,  parameter  defines  edge 
length for integration cubes.  Default is 5% of weld pool depth.
VARIABLE   
DESCRIPTION
Pi 
Parameters  defining  for  weld  pool  geometry,  depending  on 
parameter IFORM.  See Remark 4 for details. 
TX, TY, TZ 
Weld beam direction vector in global coordinates (SID2 = 0 only) 
Remarks:  
1.This keyword can be applied for solid and thermal thick shells in thermal-only and 
coupled  thermal-structural  simulations.    The  nodes  in  the  node  set  NSID1  have 
to  be  ordered,  such  that  the  node  set  defines  the  path  geometry  as  well  as  the 
direction of the trajectory.  The heat source starts at the position of the first node 
in the node set and automatically ends as soon as the last node is reached.   
By choosing nodes of the work piece for the path definition in NSID1, it can be 
ensured  that  the  heat  source  always  follows  the  movement  of  the  piece.    By 
setting  parameter  RELVEL  to  1  the  velocity  of  the  heat  source  can  even  be  de-
fined relatively to the motion of the structure.   
2.If  a  segment  set referred  to  in SID2  which  coincides  with  the  work  piece  surface, 
the weld beam direction is always orthogonal to the work piece surface.   To be 
applicable every two consecutive nodes of node set NSID1 have to be part of at 
least  one  segment.    In  case  of  more  than  one  segment  an  averaged  normal  is 
computed.  
Based on the trajectory and the weld source aiming direction, a local coordinate 
system is constructed that is centered at the root of the heat source.  By default, 
the  relative  velocity  vector  (on  the  trajectory)  of  the  heat  source  defines  the 
"forward" direction 𝒓, so material points that are approaching the heat source are 
in "front" of the beam.  The weld source aiming direction, denoted by 𝒕, is used to 
compute the weld pool depth.   The weld pool width (coordinate direction 𝒔) is 
measured normal to the relative velocity - aiming direction plane. 
The  keyword  allows  rotating  and  translating  the  coordinate  system.    First,  the 
system is rotated around the vector 𝒓 by a value given in the load curve LCROT 
resulting in a new local coordinate system (𝒓, 𝒔′, 𝒕′).  Second, the system is trans-
lated in directions 𝒕′ and  𝒔′ using LCMOV and LCLAT, respectively.   
3.The subcycling method introduces an individual time step size for the weld source 
evaluation.    Within  one  time  step  of  the  heat  transfer  solver,  NCYC  steps  are 
used  to  determine  the  energy  rate  distribution  of  the  boundary  condition.    In 
each  substep  the  geometry  of  the  weld  pool  is  updated.    Therefore,  even  with 
larger thermal time steps a relatively smooth temperature field around the weld 
source  can  be  obtained  and  a  jumping  heat  source  across  elements  can  be  sup-
pressed. 
4.This  keyword  allows  application  of  different  equivalent  heat  source  geometries, 
depending  on  the  parameter  IFORM.    The  definition  of  the  local  coordinate 
system needed for the description of the weld pool shape is discussed in Remark 
2. 
For  IFORM.EQ.1  heat is  generated  in  an ellipsoidal  region  centered  at  the  weld 
source,  and  decaying  exponentially  with  distance  according  to  the  work  of 
Goldak, Chakravarti, and Bibby [1984].  Energy rate distribution is governed by  
𝑞 =
2𝑛√𝑛𝐹𝑄
𝜋√𝜋𝑎𝑏𝑐
exp (
−𝑛𝑥2
𝑎2 ) exp (
−𝑛𝑦2
𝑏2 ) exp (
−𝑛𝑧2
𝑐2 ) 
where: 
𝐹 = {
𝑐 = {
Ff if point 𝑝 is in front of beam
Fr if point 𝑝 is behind beam
cf if point 𝑝 is in front of beam
cr if point 𝑝 is behind beam
The local coordinates of point 𝑝 are denoted by (𝑥, 𝑦, 𝑧) and it is expected that the 
sum  of  the  weighting  factors  𝐹f, 𝐹r  equals  2.    The  half-width  of  the  ellipsoid  is 
given  by  𝑎,  the  welding  depth  by  𝑏.    The  complete  set  of  parameters 
(𝑎, 𝑏, 𝑐f, 𝑐r, 𝐹f, 𝐹r, 𝑛) is input by the parameters P1 to P7, see table below. 
The  energy rate  density 𝑞  defined  by  IFORM.EQ.2  is  assumed  to  be  constant  in 
the double ellipsoidal region as defined for Goldak-type heat sources.  Its value 
is given by 
𝑞 =
3𝐹𝑄
2𝜋𝑎𝑏𝑐
with  the  same  assumptions  for  𝐹  and  𝑐  as  above.    The  set  of  parameters  conse-
quently reduces to (𝑎, 𝑏, 𝑐f, 𝑐r, 𝐹f, 𝐹r), the input of which is given by P1 to P6. 
In  contrast  to  the  above  IFORM.EQ.3  defines  an  equivalent  heat  source  with  a 
constant energy rate density on a double conical region.  The shape is defined by 
three radii 𝑟1, 𝑟2, 𝑟3and two values 𝑏1, 𝑏2 defining the heights of the two parts of 
the shape.  The respective power densities of the parts are given by 
𝑞𝑖 =
3𝐹𝑖𝑄
2 + 𝑟𝑖+1
2𝜋𝑏𝑖(𝑟𝑖
2 + 𝑟𝑖
2 )
2𝑟𝑖+1
.
Here  it  is  assumed  that  𝑖 = 1  corresponds  to  the  part  closer  to  the  weld  source.  
The input for the complete parameter set (𝑟1, 𝑟2, 𝑟3, 𝑏1, 𝑏2, 𝐹1, 𝐹2) is again defined 
by P1 to P7. 
Finally,  IFORM.EQ.4  defines  a  constant  power  density  over  a  frustum.    The 
density and the shape can easily be described using three geometrical parameters 
P1  to  P3  corresponding  to  the  radii  𝑟1(at  the  heat  source  origin)  and  𝑟2  and  the 
height 𝑏: 
𝑞 =
1 
𝑎  
𝑏  
𝑐f  
𝑐r  
𝐹f  
𝐹r  
𝑛  
IFORM 
P1 
P2 
P3 
P4 
P5 
P6 
P7 
P8 
2 + 𝑟1
2 + 𝑟2
2)
2𝑟2
𝜋𝑏(𝑟1
4 
𝑟1  
𝑟2  
𝑏1  
2 
𝑎  
𝑏  
𝑐f  
𝑐r  
𝐹f  
𝐹r  
3 
𝑟1  
𝑟2  
𝑟3  
𝑏1  
𝑏2  
𝐹f  
𝐹r
*BOUNDARY 
Purpose:    Define  a  surface  for  coupling  with  the  USA  code  [DeRuntz  1993].    The 
outward normal vectors should point into the fluid media.  The coupling with USA 
is operational in explicit transient and in implicit natural frequency analyses. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
WETDRY  NBEAM 
Type 
I 
Default 
none 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
SSID 
Segment set ID, see *SET_SEGMENT 
WETDRY 
Wet surface flag: 
EQ.0: Dry, no coupling for USA DAA analysis, or Internal fluid
coupling for USA CASE analysis 
EQ.1: Wet,  coupled  with  USA  for  DAA  analysis,  or  External
fluid coupling for USA CASE analysis 
The  number  of  nodes  touched  by  USA  Surface-of-Revolution 
(SOR) elements.  It is not necessary that the LS-DYNA model has 
beams where USA has beams (i.e., SOR elements), merely that the 
LS-DYNA  model  has  nodes  to  receive  the  forces  that  USA  will
return. 
NBEAM 
Remarks: 
The  underwater  shock  analysis  code  is  an  optional  module.    To  determine 
availability contact sales@lstc.com. 
The wet surface of 3 and 4-noded USA general boundary elements is defined in LS-
DYNA with a segment set of 4-noded surface segments, where the fourth node can 
duplicate the third node to form a triangle.  The segment normal vectors should be 
directed into the USA fluid.  If USA overlays are going to be used to reduce the size 
of the DAA matrices, the user should nonetheless define the wet surface here as if no 
overlay were being used.  If Surface-of -Revolution elements (SORs) are being used 
in USA, then NBEAM should be non-zero on one and only one card in this section. 
The wet surface defined here can cover structural elements or acoustic fluid volume 
elements, but it can not touch both types in one model.
When  running  a  coupled  problem  with  USA,  the  procedure  requires  an  additional 
input  file  of  USA  keyword  instructions.    These  are  described  in  a  separate  USA 
manual.    The  name  of  this  input  file  is  identified  on  the  command  line  with  the 
usa = flag: 
where uin is the USA keyword instruction file.
LSDYNA.USA i=inf  usa=uin
*BOUNDARY_ELEMENT_METHOD_OPTION 
Available options include: 
CONTROL 
FLOW 
NEIGHBOR 
SYMMETRY 
WAKE 
Purpose: 
incompressible fluid dynamics or fluid-structure interaction problems. 
  Define  input  parameters  for  boundary  element  method  analysis  of 
The  boundary  element  method  (BEM)  can  be  used  to  compute  the  steady  state  or 
transient fluid flow about a rigid or deformable body.  The theory which underlies the 
method    is  restricted  to  inviscid,  incompressible, 
attached fluid flow.  The method should not be used to analyze flows where shocks or 
cavitation are present. 
In  practice  the  method  can  be  successfully  applied  to  a  wider  class  of  fluid  flow 
problems than the assumption of inviscid, incompressible, attached flow would imply.  
Many flows of practical engineering significance have large Reynolds numbers (above 1 
million).    For  these  flows  the  effects  of  fluid  viscosity  are  small  if  the  flow  remains 
attached, and the assumption of zero viscosity may not be a significant limitation.  Flow 
separation does not necessarily invalidate the analysis.  If well-defined separation lines 
exist on the body, then wakes can be attached to these separation lines and reasonable 
results  can  be  obtained.    The  Prandtl-Glauert  rule  can  be  used  to  correct  for  non-zero 
Mach numbers  in a gas, so the effects of aerodynamic compressibility can be correctly 
modeled (as long as no shocks are present). 
The  BOUNDARY_ELEMENT_METHOD_FLOW  card  turns  on  the  analysis,  and  is 
mandatory.
*BOUNDARY_ELEMENT_METHOD_CONTROL 
Purpose:  Control the execution time of the boundary element method calculation.  The 
CONTROL  option  is  used  to  control  the  execution  time  of  the  boundary  element 
method  calculation,  and  the  use  of  this  option  is  strongly  recommended.    The  BEM 
calculations can easily dominate the total execution time of a LS-DYNA run unless the 
parameters on this card (especially DTBEM and/or IUPBEM) are used appropriately. 
DTBEM is used to increase the time increment between calls to the BEM routines.  This 
can  usually  be  done  with  little  loss  in  accuracy  since  the  characteristic  times  of  the 
structural dynamics and the fluid flow can differ by several orders of magnitude.  The 
characteristic  time  of  the  structural  dynamics  in  LS-DYNA  is  given  by  the  size  of  the 
smallest structural element divided by the speed of sound of its material.  For a typical 
problem this characteristic time might be equal to 1 microsecond.  Since the fluid in the 
boundary  element  method  is  assumed  to  be  incompressible  (infinite  speed  of  sound), 
the characteristic time of the fluid flow is given by the streamwise length of the smallest 
surface  in  the  flow  divided  by  the  fluid  velocity.    For  a  typical  problem  this 
characteristic time might be equal to 10 milliseconds.  For this example DTBEM might 
be set to 1 millisecond with little loss of accuracy.  Thus, for this example, the boundary 
element method would be called only once for every 1000 LS-DYNA iterations, saving 
an enormous amount of computer time. 
IUPBEM is used to increase the number of times the BEM routines are called before the 
matrix  of  influence  coefficients  is  recomputed  and  factored  (these  are  time-consuming 
procedures).  If the motion of the body is entirely rigid body motion there is no need to 
ever  recompute  and  factor  the  matrix  of  influence  coefficients  after  initialization,  and 
the execution time of the BEM can be significantly reduced by setting IUPBEM to a very 
large  number.    For  situations  where  the  structural  deformations  are  modest  an 
intermediate value (e.g., 10) for IUPBEM can be used. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LWAKE 
DTBEM 
IUPBEM 
FARBEM 
Type 
I 
Default 
50 
F 
0. 
I 
F 
100 
2.0 
Remark 
1
DESCRIPTION
Number of elements in the wake of lifting surfaces.  Wakes must
be defined for all lifting surfaces. 
Time  increment  between  calls  to  the  boundary  element  method.
The  fluid  pressures  computed  during  the  previous  call  to  the
BEM will continue to be used for subsequent LS-DYNA iterations 
until a time increment of DTBEM has elapsed. 
The  number  of  times  the  BEM  routines  are  called  before  the 
matrix of influence coefficients is recomputed and refactored. 
Nondimensional  boundary  between  near-field  and  far-field 
calculation of influence coefficients. 
  VARIABLE   
LWAKE 
DTBEM 
IUPBEM 
FARBEM 
Remarks: 
1.  Wakes  convect  with  the  free-stream  velocity.    The  number  of  elements  in  the 
wake should be set to provide a total wake length equal to 5-10 times the char-
acteristic streamwise length of the lifting surface to which the wake is attached.  
Note that each wake element has a streamwise length equal to the magnitude of 
the  free  stream  velocity  multiplied  by  the  time  increment  between  calls  to  the 
boundary  element  method  routines.    This  time  increment  is  controlled  by 
DTBEM. 
2.  The most accurate results will be obtained with FARBEM set to 5 or more, while 
values as low as 2 will provide slightly reduced accuracy with a 50% reduction 
in the time required to compute the matrix of influence coefficients.
*BOUNDARY_ELEMENT_METHOD_FLOW 
Purpose:    Turn  on  the  boundary  element  method  calculation,  specify  the  set  of  shells 
which define the surface of the bodies of interest, and specify the onset flow. 
The  *BOUNDARY_ELEMENT_METHOD_FLOW  card  turns  on  the  BEM  calculation.  
This  card  also  identifies  the  shell  elements  which  define  the  surfaces  of  the  bodies  of 
interest,  and  the  properties  of  the  onset  fluid  flow.    The  onset  flow  can  be  zero  for 
bodies which move through a fluid which is initially at rest. 
  Card 1 
1 
Variable 
SSID 
Type 
I 
2 
VX 
F 
3 
VY 
F 
4 
VZ 
F 
5 
6 
7 
8 
RO 
PSTATIC  MACH 
F 
F 
Default 
none 
none 
none 
none 
none 
0. 
Remark 
1 
2 
F 
0. 
3 
  VARIABLE   
SSID 
DESCRIPTION
Shell set ID for the set of shell elements which define the surface
of  the  bodies  of  interest  .    The  nodes  of  these 
shells  should  be  ordered  so  that  the  shell  normals  point  into  the
fluid. 
VX, VY, VZ 
x, y, and z components of the free-stream fluid velocity. 
RO 
Fluid density. 
PSTATIC 
Fluid static pressure. 
MACH 
Free-stream Mach number. 
Remarks: 
1. 
It  is  recommended  that  the  shell  segments  in  the  SSID  set  use  the  NULL 
material .  This will provide for the display of fluid pressures 
in the post-processor.  For triangular shells the 4th node number should be the 
same  as  the  3rd  node  number.    For  fluid-structure  interaction  problems  it  is 
recommended  that  the  boundary  element  shells  use  the  same  nodes  and  be
coincident  with  the  structural  shell  elements  (or  the  outer  face  of  solid  ele-
ments) which define the surface of the body.  This approach guarantees that the 
boundary  element  segments  will  move  with  the  surface  of  the  body  as  it  de-
forms. 
2.  A pressure of PSTATIC is applied uniformly to all segments in the segment set.  
If the body of interest is hollow, then PSTATIC should be set to the free-stream 
static pressure minus the pressure on the inside of the body. 
3.  The  effects  of  subsonic  compressibility  on  gas  flows  can  be  included  using  a 
non-zero value for MACH.  The pressures  which arise from the fluid flow are 
increased using the Prandtl-Glauert compressibility correction.  MACH should 
be set to zero for water or other liquid flows.
*BOUNDARY_ELEMENT_METHOD_NEIGHBOR 
Purpose:  Define the neighboring elements for a given boundary element segment. 
The  pressure  at  the  surface  of  a  body  is  determined  by  the  gradient  of  the  doublet 
distribution on the surface .  The “Neighbor Array” 
is  used  to  specify  how  the  gradient  is  computed  for  each  boundary  element  segment.  
Ordinarily, the Neighbor Array is set up automatically by LS-DYNA, and no user input 
is required.  The NEIGHBOR option is provided for those circumstances when the user 
desires to define this array manually. 
Elements Cards.  The next “*” card terminates the input. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NELEM 
NABOR1  NABOR2  NABOR3  NABOR4 
Type 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
NELEM 
Element number. 
NABOR1 
Neighbor for side 1 of NELEM. 
NABOR2 
Neighbor for side 2 of NELEM. 
NABOR3 
Neighbor for side 3 of NELEM. 
NABOR4 
Neighbor for side 4 of NELEM. 
Remarks: 
Each boundary element has 4 sides (Figure 6-1).  Side 1 connects the 1st and 2nd nodes, 
side 2 connects the 2nd and 3rd nodes, etc.  The 4th side is null for triangular elements.
node 4
side 3
node 3
side 4
node 1
segment(j)
side 1
side 2
node 2
Figure 6-1.  Each segment has 4 sides. 
For most elements the specification of neighbors is straightforward.  For the typical case 
a quadrilateral element is surrounded by 4 other elements, and the neighbor array is as 
shown in Figure 6-2. 
neighbor(3, j)
side 3
neighbor(4, j)
side 4
segment(j)
side 1
side 2
neighbor(2, j)
neighbor(1, j)
Figure 6-2.  Typical neighbor specification. 
There  are  several  situations  for  which  the  user  may  desire  to  directly  specify  the 
neighbor  array  for  certain  elements.    For  example,  boundary  element  wakes  result  in 
discontinuous  doublet  distributions,  and  neighbors  which  cross  a  wake  should  not  be 
used.  Figure 6-3 illustrates a situation where a wake is attached to side 2 of segment j.  
For  this  situation  two  options  exist.    If  neighbor(2,j)  is  set  to  zero,  then  a  linear 
computation  of  the  gradient  in  the  side  2  to  side  4  direction  will  be  made  using  the 
difference between the doublet strengths on segment j and segment neighbor(4,j).  This 
is the default setup used by LS-DYNA when no user input is provided.  By specifying 
neighbor(2,j) as a  negative number a more accurate quadratic curve fit will be  used to 
compute  the  gradient.    The  curve  fit  will  use  segment  j,  segment  neighbor(4,j),  and 
segment -neighbor(2,j); which is located on the opposite side of segment neighbor(4,j) as 
segment j.
-neighbor(2, j)
neighbor(4, j)
side 3
side 4
segment(j)
side 1
side 2
Figure  6-3.    If  neighbor(2,j)  is  a  negative  number  it  is  assumed  to  lie  on  the 
opposite side of neighbor(4,j) as segment j. 
Another  possibility  is  that  no  neighbors  at  all  are  available  in  the  side  2  to  side  4 
direction.    In  this  case  both  neighbor(2,j)  and  neighbor(4,j)  can  be  set  to  zero,  and  the 
gradient in that direction will be assumed to be zero.  This option should be used with 
caution,  as  the  resulting  fluid  pressures  will  not  be  accurate  for  three-dimensional 
flows.  However, this option is occasionally useful where quasi-two dimensional results 
are  desired.    All  of  the  above  options  apply  to  the  side  1  to  side  3  direction  in  the 
obvious ways. 
For  triangular  boundary  elements  side  4  is  null.    Gradients  in  the  side  2  to  side  4 
direction  can  be  computed  as  described  above  by  setting  neighbor(4,j)  to  zero  for  a 
linear derivative computation (this is the default setup used by LS-DYNA when no user 
input  is  provided)  or  to  a  negative  number  to  use  the  segment  on  the  other  side  of 
neighbor(2,j) and a quadratic curve fit.  There may also be another triangular segment 
which can be used as neighbor(4,j) . 
neighbor(4, j)
segment(j)
side 2
Figure 6-4.  Sometimes another triangular boundary element segment can be
used as neighbor (4,j). 
The  rules  for  computing  the  doublet  gradient  in  the  side  2  to  side  4  direction  can  be 
summarized as follows (the side 1 to side 3 case is similar):
NABOR2 
NABOR4 
Doublet Gradient Computation 
GT.0 
GT.0 
Quadratic fit using elements j, 
NABOR2, and NABOR4. 
LT.0 
GT.0 
GT.0 
LT.0 
Quadratic fit using elements j, -NAB-
OR2, and NABOR4.  -NABOR2 is 
assumed to lie on the opposite side of 
NABOR4 as segment j . 
Quadratic fit using elements j, 
NABOR2, and -NABOR4.  -NABOR4 
is assumed to lie on the opposite side 
of NABOR2 as segment j. 
EQ.0 
GT.0 
GT.0 
EQ.0 
EQ.0 
EQ.0 
Linear fit using elements j and 
NABOR4. 
Linear fit using elements j and 
NABOR2. 
Zero gradient. 
Table 3.1  Surface pressure computation for element j.
*BOUNDARY_ELEMENT_METHOD_SYMMETRY 
Purpose:    To  define  a  plane  of  symmetry  for  the  boundary  element  method.    The 
SYMMETRY option can be used to reduce the time and memory required for symmetric 
configurations.    For  these  configurations  the  reduction  in  the  number  of  boundary 
elements by a factor of 2 will reduce the memory used by the boundary element method 
by  a  factor  of  4,  and  will  reduce  the  computer  time  required  to  factor  the  matrix  of 
influence coefficients by a factor of 8.  Only 1 plane of symmetry can be defined. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  BEMSYM 
Type 
Default 
I 
0 
  VARIABLE   
DESCRIPTION
BEMSYM 
Defines symmetry plane for boundary element method. 
EQ.0: no symmetry plane is defined 
EQ.1: x = 0 is a symmetry plane 
EQ.2: y = 0 is a symmetry plane 
EQ.3: z = 0 is a symmetry plane
*BOUNDARY_ELEMENT_METHOD_WAKE 
Purpose:    To  attach  wakes  to  the  trailing  edges  of  lifting  surfaces.    Wakes  should  be 
attached to boundary elements at the trailing edge of a lifting surface (such as a wing, 
propeller  blade,  rudder,  or  diving  plane).    Wakes  should  also  be  attached  to  known 
separation lines when detached flow is known to exist (such as the sharp leading edge 
of  a  delta  wing  at  high  angles  of  attack).    Wakes  are  required  for  the  correct 
computation  of  surface  pressures  for  these  situations.    As  described  above,  two 
segments on opposite sides of a wake should never be used as neighbors. 
Element Cards.  (The next “*” card terminates the input.)  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NELEM 
NSIDE 
Type 
I 
I 
Default 
none 
none 
Remark 
1 
  VARIABLE   
DESCRIPTION
NELEM 
Element number to which a wake is attached. 
NSIDE 
The side of NELEM to which the wake is attached .
This should be the "downstream" side of NELEM. 
Remarks: 
1.  Normally two elements meet at a trailing edge (one on the "upper" surface and 
one  on  the  "lower"  surface).    The  wake  can  be  attached  to  either  element,  but 
not to both.
The *CASE command provides a way of running multiple LS-DYNA analyses (or cases) 
sequentially  by  submitting  a  single  input  file.      When  *CASE  commands  are  used  to 
define  multiple  cases,  some  portions  of  the  input  will  be  shared  by  some  or  all  of  the 
cases  and  other  portions  will  be  unique  to  each  case.    Because  the  cases  are  run 
sequentially, the results from one case, e.g., a dynain file, can be used in the analysis of 
a  different,  subsequent  case.    Each  case  creates  a  unique  set  of  output  file  names  by 
prepending “casen.” to the default file name, e.g., case101.d3plot, case102.glstat.  
When  the  *CASE  keyword  appears  in  an  input  deck,  it  becomes  necessary  to  append 
the  word  “CASE”  to  the  LS-DYNA  execution  line.    For  example,  an  SMP  LS-DYNA 
execution line might look something like 
path_to_ls-dyna i=input.k ncpu=-4 CASE 
An MPP LS-DYNA execution line might look something like  
mpirun –np 4  path_to_mpp971  i=input.k CASE 
*CASE_{OPTION} 
Available options include: 
<BLANK> 
BEGIN_N 
END_N 
Purpose:  Define a series of cases and perhaps subcases.  The options *CASE_BEGIN_n 
and  *CASE_END_n  appear  in  pairs  and  n  is  a  numeric  ID  of  a  subcase.    Subcase  IDs 
may  be  referenced  by the  *CASE  command  in  defining  a  case.    In other  words,  a  case 
may  consist  of  one  or  more  subcases.    All  keywords  appearing  between  *CASE_BE-
GIN_n and *CASE_END_n comprise subcase n.  If no *CASE command is defined, then 
subcases defined by *CASE_BEGIN_n and *CASE_END_n then become cases.  *CASE_-
BEGIN/*CASE_END  can  be  nested,  overlapped,  and  disjointed.    Examples  below 
demonstrate the use of these options. 
An alternative way of defining subcases is by appending the string “CID = n” to the end 
of any keyword command.  Any keyword so tagged will then be active only for those 
cases that reference subcase n.  There can be more than one space between the keyword 
and “CID = n”.   
Any keyword in the input deck not associated with a subcase is active for all cases.
GIN/*CASE_END. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CASEID 
JOBID 
Type 
I 
C 
Default 
none 
none 
Command Line Argument Cards.  Command line cards set additional command line 
arguments for the case CASEID .  Include as many as needed, or as 
few  as  none.    Command  line  cards  end  when  the  first  character  of  the  next  card  is 
numeric. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
COMMANDS 
A 
Not Required 
Subcase  ID  Cards.    Define  active  subcase  IDs  for  case  CASEID  . 
These cards continue until the next keyword (“*”) card. 
  Card 3 
1 
2 
Variable 
SCID1 
SCID2 
Type 
I 
I 
3 
… 
I 
4 
… 
I 
5 
… 
I 
6 
… 
I 
7 
… 
I 
8 
… 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
CASEID 
Identification number for case.
VARIABLE   
JOBID 
DESCRIPTION
Optional string (no spaces) to be used as the jobid for this case.  If
no  JOBID  is  specified,  the  string  CASEXX  is  used,  where  XX  is
the CASEID in field 1 
*CASE 
COMMANDS 
Command line arguments. 
SCIDn 
Subcase ID active for case CASEID. 
Remarks: 
1. 
2. 
3. 
If no *CASE keyword appears, subcases defined with *CASE_BEGIN/*CASE_-
END commands become cases and  *CASE_BEGIN can optionally be followed 
by extra command line arguments. 
If  no  *CASE  keyword  appears,  it  is  an  error  to  append  “CID = n”  to  any 
keyword.  
If  multiple  *CASE  or  *CASE_BEGIN  keywords  appear  that  have  the  same  ID, 
their command line arguments and active commands are merged.   
4.  The *CASE or *CASE_BEGIN keywords cannot be used within an include (*IN-
CLUDE) file. 
Example 1: 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$ Define case 101 which includes subcase 1. 
$ Define case 102 which includes subcase 4. 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
*CASE 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7 
$   CASEID 
       101 JOBID_FOR_CASE101 
MEMORY=20M 
1 
$       
*CASE 
$   CASEID 
       102      
MEMORY=20M  NCYCLE=1845 
4 
$ 
*TITLE  CID=1 
THIS IS THE TITLE FOR CASE 101 
$ 
*TITLE  CID=4 
THIS IS THE TITLE FOR CASE 102 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  Illustrate overlapping subcases. 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
*CASE_BEGIN_5 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....> 
*DATABASE_BINARY_D3THDT 
1.e-5 
*CASE_BEGIN_3 
*DATABASE_NODOUT 
1.e-5 
*CASE_END_5 
*DATABASE_ELOUT 
1.e-5 
*CASE_END_3 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
Example 2 above will generate d3thdt and nodout for CID = 5, and nodout and elout for 
CID = 3.
*COMMENT 
All input that falls between a *COMMENT command and the subsequent line of input 
that  has  an  asterisk  in  the  first  column  thereby  signaling  the  start of  another  keyword 
command,  is  not  acted  on  by  LS-DYNA.    This  provides  a  convenient  way  to  interject 
multiple, successive lines of commentary anywhere inside an input deck.   
*COMMENT  also  provides  a  convenient  way  to  comment  out  an  exisiting  keyword 
command and all its associated input data as shown in an example below. 
Lines of input that are deactivated by *COMMENT are echoed on the screen and to the 
messag and d3hsp files. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
COMMENT 
A 
none 
  VARIABLE   
DESCRIPTION 
COMMENT 
Any comment line. 
Example: 
In this excerpt from an input deck, 5 lines of comments including blank lines, are added 
to the input deck. 
*KEYWORD 
*COMMENT 
Units of this model are mks. 
Input prepared by John Doe. 
Input checked by Jane Doe. 
*CONTROL_TERMINATION 
1.E-02 
⋮
*COMMENT 
In  this  excerpt  from  an  input  deck,  a  contact  is  disabled  by  inserting  *COMMENT 
command before the contact keyword command. 
⋮  
*COMMENT  *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_ID 
$#     cid                                                                 title 
         1 
$#    ssid      msid     sstyp     mstyp    sboxid    mboxid       spr       mpr 
1,2,0,3 
$#      fs        fd        dc        vc       vdc    penchk        bt        dt 
0.2 
$#     sfs       sfm       sst       mst      sfst      sfmt       fsf       vsf 
$#    soft    sofscl    lcidab    maxpar     sbopt     depth     bsort    frcfrq 
         2 
*SET_SEGMENT 
$#     sid       da1       da2       da3       da4    solver 
         1     0.000     0.000     0.000     0.000MECH 
$#      n1        n2        n3        n4        a1        a2        a3        a4 
      2842       626      3232      3242     0.000     0.000     0.000     0.000 
      2846      2842       627      2843     0.000     0.000     0.000     0.000 
⋮
The keyword *COMPONENT provides a way of incorporating specialized components 
and  features.    The  keyword  control  cards  in  this  section  are  defined  in  alphabetical 
order: 
*COMPONENT_GEBOD_OPTION 
*COMPONENT_GEBOD_JOINT_OPTION 
*COMPONENT_HYBRIDIII 
*COMPONENT_HYBRIDIII_JOINT_OPTION
*COMPONENT_GEBOD 
Purpose:    Generate  a  rigid  body  dummy  based  on  dimensions  and  mass  properties 
from  the  GEBOD  database.    The  motion  of  the  dummy  is  governed  by  equations 
integrated  within  LS-DYNA  separately  from  the  finite  element  model.    Default  joint 
characteristics  (stiffness’s,  stop  angles,  etc.)  are  set  internally  and  should  give 
reasonable  results,  however, they  may  be  altered  using the  *COMPONENT_GEBOD_-
JOINT command.  Contact between the segments of the dummy and the finite element 
model  is  defined  using  the  *CONTACT_GEBOD  command.    The  use  of  a  positioning 
file is essential with this feature, see Appendix N for further details. 
OPTION specifies the human subject type.  The male and female types represent adults 
while the child is genderless. 
MALE 
FEMALE 
CHILD 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DID 
UNITS 
SIZE 
Type 
I 
I 
F 
Default 
none 
none 
none 
  Card 2 
Variable 
1 
VX 
Type 
F 
Default 
0. 
2 
VY 
F 
0. 
3 
VZ 
F 
0. 
4 
GX 
F 
0. 
5 
GY 
F 
0. 
6 
GZ 
F 
0. 
7 
8 
  VARIABLE   
DESCRIPTION
DID 
Dummy ID.  A unique number must be specified.
VARIABLE   
DESCRIPTION
UNITS 
System of units used in the finite element model. 
EQ.1:  lbf × sec2/in - inch - sec 
EQ.2:  kg - meter - sec 
EQ.3:  kgf × sec2/mm - mm - sec 
EQ.4:  metric ton - mm - sec 
EQ.5:  kg - mm - msec 
SIZE 
Size  of  the  dummy.    This  represents  a  combined  height  and
weight  percentile  ranging  from 0  to  100  for  the  male  and  female
types.  For the child the number of months of age is input with an
admissible range from 24 to 240. 
VX, VY, VZ 
Initial velocity of the dummy in the global x, y and z directions. 
GX, GY, GZ 
Global  x,  y,  and  z  components  of  gravitational  acceleration
applied to the dummy. 
Example: 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *COMPONENT_GEBOD_MALE 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  A 50th percentile male dummy with the ID number of 7 is generated in the 
$  lbf*sec^2-inch-sec system of units.  The dummy is given an initial velocity of 
$  616 in/sec in the negative x direction and gravity acts in the negative z 
$  direction with a value 386 in/sec^2.  
$ 
*COMPONENT_GEBOD_MALE 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      did     units      size 
         7         1        50 
$       vx        vy        vz        gx        gy        gz 
      -616         0         0         0         0      -386 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$
*COMPONENT_GEBOD_JOINT_OPTION 
Purpose:  Alter the joint characteristics of a GEBOD rigid body dummy.   Setting a joint 
parameter  value  to  zero  retains  the  default  value  set  internally.    See  Appendix  N  for 
further details. 
The following options are available. 
PELVIS 
WAIST 
LOWER_NECK 
UPPER_NECK 
LEFT_SHOULDER 
RIGHT_SHOULDER 
LEFT_ELBOW 
RIGHT_ELBOW 
LEFT_HIP 
RIGHT_HIP 
LEFT_KNEE 
RIGHT_KNEE 
LEFT_ANKLE 
RIGHT_ANKLE 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DID 
LC1 
LC2 
LC3 
SCF1 
SCF2 
SCF3 
Type 
F 
I 
I 
I 
F 
F 
F 
  VARIABLE   
DESCRIPTION
DID 
LCi 
SCFi 
Dummy ID, see *COMPONENT_GEBOD_OPTION. 
Load  curve  ID  specifying  the  loading  torque  versus  rotation  (in
radians) for the ith degree of freedom of the joint.   
Scale  factor  applied  to  the  load  curve  of  the  ith  joint  degree  of 
freedom.
Card 2 
Variable 
1 
C1 
Type 
F 
2 
C2 
F 
3 
C3 
F 
4 
5 
6 
7 
8 
NEUT1 
NEUT2 
NEUT3 
F 
F 
F 
  VARIABLE   
DESCRIPTION
Ci 
Linear  viscous  damping  coefficient  applied  to  the  ith  DOF  of  the 
joint.    Units  are  torque ×  time/radian,  where  the  units  of  torque 
and  time  depend  on  the  choice  of  UNITS  in  card  1  of  *COMPO-
NENT_GEBOD_OPTION. 
NEUTi 
Neutral angle (degrees) of joint's ith DOF. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LOSA1 
HISA1 
LOSA2 
HISA2 
LOSA3 
HISA3 
Type 
F 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
LOSAi 
HISAi 
Value of the low stop angle (degrees) for the ith DOF of this joint. 
Value of the high stop angle (degrees) for the ith DOF of this joint.
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
UNK1 
UNK2 
UNK3 
Type 
F 
Default 
0. 
F 
0. 
F 
0.
DESCRIPTION
Unloading  stiffness  (torque/radian)  for the ith  degree of  freedom 
of  the  joint.    This  must  be  a  positive  number.    Units  of  torque
depend on the choice of UNITS in card 1 of *COMPONENT_GE-
BOD_OPTION. 
  VARIABLE   
UNKi 
Example 1: 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *COMPONENT_GEBOD_JOINT_LEFT_SHOULDER 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  The damping coefficients applied to all three degrees of freedom of the left 
$  shoulder of dummy 7 are set to 2.5.  All other characteristics of this joint 
$  remain set to the default value. 
$ 
*COMPONENT_GEBOD_JOINT_LEFT_SHOULDER 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      did       lc1       lc2       lc3      scf1      scf2      scf3 
         7         0         0         0         0         0         0 
$       c1        c2        c3     neut1     neut2     neut3 
       2.5       2.5       2.5         0         0         0 
$    losa1      hisa1    losa2     hisa2     losa3     hisa3 
         0         0         0         0         0         0 
$     unk1      unk2      unk3 
         0         0         0 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
Example 2: 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *COMPONENT_GEBOD_JOINT_WAIST 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Load curve 8 gives the torque versus rotation relationship for the 2nd DOF 
$  (lateral flexion) of the waist of dummy 7.  Also, the high stop angle of the 
$  1st DOF (forward flexion) is set to 45 degrees.  All other characteristics  
$  of this joint remain set to the default value. 
$ 
*COMPONENT_GEBOD_JOINT_WAIST 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      did       lc1       lc2       lc3      scf1      scf2      scf3 
         7         0         8         0         0         0         0 
$       c1        c2        c3     neut1     neut2     neut3 
         0         0         0         0         0         0 
$    losa1     hisa1     losa2     hisa2     losa3     hisa3 
         0        45         0         0         0         0 
$     unk1      unk2      unk3 
         0         0         0 
$
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
*COMPONENT_HYBRIDIII 
Purpose:    Define  a  HYBRID  III  dummy.    The  motion  of  the  dummy  is  governed  by 
equations  integrated  within  LS-DYNA  separately  from  the  finite  element  model.    The 
dummy  interacts  with  the  finite  element  structure  through  contact  interfaces.    Joint 
characteristics  (stiffnesses,  damping,  friction,  etc.)  are  set  internally  and  should  give 
reasonable results, however, they may be altered using the *COMPONENT_HYBRIDI-
II_JOINT  command.    Joint  force  and  moments  can  be  written  to  an  ASCII  file  . 
  Card 1 
1 
2 
3 
4 
Variable 
DID 
SIZE 
UNITS 
DEFRM 
Type 
I 
I 
I 
Default 
none 
none 
none 
I 
1 
8 
5 
VX 
F 
0. 
6 
VY 
F 
0. 
7 
VZ 
F 
0. 
  VARIABLE   
DESCRIPTION
DID 
SIZE 
Dummy ID.  A unique number must be specified. 
Size of dummy. 
EQ.1:  5th percentile adult 
EQ.2:  50th percentile adult 
EQ.3:  95th percentile adult 
NOTE: If  negative  then  the  best  of  currently  available  joint
properties are applied. 
UNITS 
System of units used in the finite element model. 
EQ.1:  lbf × sec2/in - inch - sec 
EQ.2:  kg - meter - sec 
EQ.3:  kgf × sec2/mm - mm - sec 
EQ.4:  metric ton - mm - sec 
EQ.5:  kg - mm - msec
VARIABLE   
DESCRIPTION
DEFRM 
Deformability type. 
EQ.1:  all dummy segments entirely rigid 
EQ.2:  deformable abdomen (low density foam, mat #57) 
EQ.3:  deformable jacket (low density foam, mat #57) 
EQ.4:  deformable headskin (viscoelastic, mat #6) 
EQ.5:  deformable abdomen/jacket 
EQ.6:  deformable jacket/headskin 
EQ.7:  deformable abdomen/headskin 
EQ.8:  deformable abdomen/jacket/headskin 
VX, VY, VZ 
Initial velocity of the dummy in the global x, y and z directions. 
  Card 2 
Variable 
1 
HX 
Type 
F 
Default 
0. 
2 
HY 
F 
0. 
3 
HZ 
F 
0. 
4 
RX 
F 
0. 
5 
RY 
F 
0. 
6 
RZ 
F 
0. 
7 
8 
  VARIABLE   
DESCRIPTION
HX, HY, HZ 
Initial global x, y, and z coordinate values of the H-point. 
RX, RY, RZ 
Initial  rotation  of  dummy  about  the  H-point  with  respect  to  the 
global x, y, and z axes (degrees). 
Example 1: 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *COMPONENT_HYBRIDIII 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  A 50th percentile adult rigid HYBRID III dummy with an ID number of 7 is defined 
$  in the lbf*sec^2-inch-sec system of units.  The dummy is assigned an initial 
$  velocity of 616 in/sec in the negative x direction.  The H-point is initially  
$  situated at (x,y,z)=(38,20,0) and the dummy is rotated 18 degrees about the  
$  global x-axis. 
$
*COMPONENT_HYBRIDIII 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      did    .  size     units     defrm        vx        vy        vz 
         7         2         1         1     -616.        0.        0.         
$       hx        hy        hz        rx        ry        rz 
       38.       20.        0.       18.        0.        0. 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
*COMPONENT_HYBRIDIII_JOINT_OPTION 
Purpose:    Alter  the  joint  characteristics  of  a  HYBRID  III  dummy.    Setting  a  joint 
parameter  value  to  zero  retains  the  default  value  set  internally.    Joint  force  and 
moments  can  be  written  to  an  ASCII  file  .    Further  details 
pertaining to the joints are found in the Hybrid III Dummies section of Appendix N. 
The following options are available: 
LUMBAR 
RIGHT_ELBOW 
RIGHT_KNEE 
LOWER_NECK 
LEFT_WRIST 
LEFT_ANKLE 
UPPER_NECK 
RIGHT_WRIST 
RIGHT_ANKLE 
LEFT_SHOULDER 
LEFT_HIP 
STERNUM 
RIGHT_SHOULDER 
RIGHT_HIP 
LEFT_KNEE_SLIDER 
LEFT_ELBOW 
LEFT_KNEE 
RIGHT_KNEE_SLIDER 
  Card 1 
1 
Variable 
DID 
Type 
F 
  Card 2 
Variable 
1 
C1 
2 
Q1 
F 
2 
3 
Q2 
F 
3 
4 
Q3 
F 
4 
5 
6 
7 
8 
FRIC 
F 
5 
6 
7 
8 
ALO1 
BLO1 
AHI1 
BHI1 
QLO1 
QHI1 
SCLK1 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Leave blank if joint has only one degree of freedom.  
  Card 3 
Variable 
1 
C2 
2 
3 
4 
5 
6 
7 
8 
ALO2 
BLO2 
AHI2 
BHI2 
QLO2 
QHI2 
SCLK2 
Type 
F 
F 
F 
F 
F 
F 
F
Leave blank if the joint has only two degrees of freedom.  
  Card 4 
Variable 
1 
C3 
2 
3 
4 
5 
6 
7 
8 
ALO3 
BLO3 
AHI3 
BHI3 
QLO3 
QHI3 
SCLK3 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
Dummy ID, see *COMPONENT_HYBRIDIII 
Initial value of the joint's ith degree of freedom.  Units of degrees 
are  defined  for  rotational  DOF.    See  Appendix  N  for  a  listing  of
the applicable DOF. 
Friction load on the joint. 
Linear  viscous  damping  coefficient  applied  to  the  ith  DOF  of  the 
joint. 
Linear coefficient for the low regime spring of the joint's ith DOF. 
Cubic coefficient for the low regime spring of the joint's ith DOF. 
Linear coefficient for the high regime spring of the joint's ith DOF.
Cubic coefficient for the high regime spring of the joint's ith DOF. 
Value at which the low regime spring definition becomes active. 
Value at which the high regime spring definition becomes active. 
Scale  value  applied  to  the  stiffness  of  the 
(default = 1.0). 
joint's  ith  DOF 
DID 
Qi 
FRIC 
Ci 
ALOi 
BLOi 
AHIi 
BHIi 
QLOi 
QHIi 
SCLKi 
Example: 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *COMPONENT_HYBRIDIII_JOINT_LEFT_ANKLE 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  The damping coefficients applied to all three degrees of freedom of the left 
$  ankle of dummy 7 are set to 2.5.  All other characteristics of this joint 
$  remain set to the default value.  The dorsi-plantar flexion angle is set to 
$  20 degrees.
$ 
*COMPONENT_HYBRIDIII_JOINT_LEFT_ANKLE 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      did        q1        q2        q3      fric 
         7         0       20.         0         0         0 
$       c1      alo1      blo1      ahi1      bhi1      qlo1      qhi1 
       2.5         0         0         0         0         0         0 
$       c2      alo2      blo2      ahi2      bhi2      qlo2      qhi2 
       2.5         0         0         0         0         0         0 
$      2.5      alo3      blo3      ahi3      bhi3      qlo3      qhi3
The  keyword  *CONSTRAINED  provides  a  way  of  constraining  degrees  of  freedom  to 
move  together  in  some  way.    The  keyword  cards  in  this  section  are  defined  in 
alphabetical order: 
*CONSTRAINED_ADAPTIVITY 
*CONSTRAINED_BEAM_IN_SOLID 
*CONSTRAINED_BUTT_WELD 
*CONSTRAINED_COORDINATE_{OPTION} 
*CONSTRAINED_EULER_IN_EULER 
*CONSTRAINED_EXTRA_NODES_OPTION 
*CONSTRAINED_GENERALIZED_WELD_OPTION_{OPTION} 
*CONSTRAINED_GLOBAL 
*CONSTRAINED_INTERPOLATION_{OPTION} 
*CONSTRAINED_INTERPOLATION_SPOTWELD 
*CONSTRAINED_JOINT_OPTION_{OPTION}_{OPTION}_{OPTION} 
*CONSTRAINED_JOINT_COOR_OPTION_{OPTION}_{OPTION}_{OPTION} 
*CONSTRAINED_JOINT_STIFFNESS_OPTION 
*CONSTRAINED_JOINT_USER_FORCE 
*CONSTRAINED_LAGRANGE_IN_SOLID 
*CONSTRAINED_LINEAR_GLOBAL 
*CONSTRAINED_LINEAR_LOCAL 
*CONSTRAINED_LOCAL 
*CONSTRAINED_MULTIPLE_GLOBAL 
*CONSTRAINED_NODAL_RIGID_BODY_{OPTION}_{OPTION} 
*CONSTRAINED_NODE_INTERPOLATION
*CONSTRAINED_NODE_TO_NURBS_PATCH 
*CONSTRAINED_POINTS 
*CONSTRAINED_RIGID_BODIES 
*CONSTRAINED_RIGID_BODY_INSERT 
*CONSTRAINED_RIGID_BODY_STOPPERS 
*CONSTRAINED_RIVET_{OPTION} 
*CONSTRAINED_SHELL_TO_SOLID 
*CONSTRAINED_SPLINE 
*CONSTRAINED_SPOTWELD_{OPTION}_{OPTION} 
*CONSTRAINED_SPR2 
*CONSTRAINED_TIEBREAK 
*CONSTRAINED_TIED_NODES_FAILURE
*CONSTRAINED_ADAPTIVITY 
Purpose:    Constrains  a  node  to  the  midpoint  along  an  edge  of  an  element.    This 
keyword  is  automatically  created  by  LS-DYNA  during  an  h-adaptive  simulation 
involving 3-D shells.  
  Card 1 
Variable 
1 
SN 
2 
3 
4 
5 
6 
7 
8 
MN1 
MN2 
Type 
I 
I 
I 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION
SN 
MN1 
MN2 
Slave  node.    This  is  the  node  constrained  at  the  midpoint  of  an
edge of an element. 
The node at one end of an element edge. 
The node at the other end of that same element edge.
*CONSTRAINED_BEAM_IN_SOLID_{OPTION} 
Available options include: 
<BLANK> 
ID 
TITLE 
Purpose:    This  keyword  constrains  beam  structures  to  move  with  Lagrangian 
solids/thick  shells,  which  serve  as  the  master  component.    This  keyword  constrains 
both acceleration and velocity.  This feature is intended to sidestep certain limitations in 
the CTYPE = 2 implementation in *CONSTRAINED_LAGRANGE_IN_SOLID.  Notable 
features of this keyword include: 
1.  CDIR = 1  feature.  With  the  CDIR = 1  option  coupling  occurs  only  in  the 
normal  directions.    This  coupling  allows  for  releasing  the  constraints  along 
beam axial direction. 
2.  Axial  coupling  force.  Debonding  processes  can  be  modeled  with  a  user 
defined function or user provided subroutine giving the axial shear force based 
on  the  slip  between  rebar  nodes  and  concrete  solid  elements.    This  feature  is 
invoked  by  setting  AXFOR  flag  to  a  negative  integer  which  refers  to  the  *DE-
FINE_FUNCTION ID or a number greater than 1000.  In the latter case, first we 
need to modify the subroutine rebar_bondslip_get_getforce() in dyn21.F to add 
in  one  or  more  debonding  laws;  each  tagged  with  a  “lawid”.    Then  we  could 
specify which debonding law to use with the AXFOR flag.  AXFOR value great-
er than 1000 will call the user subroutine and pass AXFOR in as “lawid”.  CDIR 
has to be set to 1 in this case to release the axial constraints. 
3.  NCOUP  feature.  Coupling  not  only  at  nodes,  but  also  at  multiple  coupling 
points in between the two beam element nodes.  Please note, the previous im-
plementation  done  in  *CONSTRAINED_LAGRANGE_IN_SOLID  CTYPE  2 
causes errors in energy balance. 
4.  Tetrahedral and pentahedra solid elements are supported. They are treated 
as degenerated hexahedra in CTYPE2 implementation. 
5.  Velocity/Fixed  boundary  condition.    The  CTYPE  2  implementation  failed  to 
constrain beam nodes that were buried inside elements whose nodes had veloc-
ity/fixed boundary conditions prescribed. 
6.  Optimized  Sorting.    Sorting  subroutine  is  optimized  for  larger  problems  to 
achieve better performance and less memory usage.
If  a  title  is  not  defined,  LS-DYNA  will  automatically  create  an  internal  title  for  this 
coupling definition.  
Title Card.  Additional card for TITLE and ID keyword options. 
Title 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
COUPID 
Type 
I 
TITLE 
A70 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SLAVE  MASTER 
SSTYP 
MSTYP 
NCOUP 
CDIR 
I 
0 
7 
I 
0 
8 
5 
6 
Type 
I 
I 
Default 
none 
none 
  Card 2 
1 
2 
I 
0 
3 
I 
0 
4 
Variable 
START 
END 
AXFOR 
Type 
Default 
F 
0 
F 
1010 
I 
0 
  VARIABLE   
COUPID 
DESCRIPTION
Coupling  (card)  ID  number  (I10).    If  not  defined,  LS-DYNA  will 
assign  an  internal  coupling  ID  based  on the  order of  appearance
in the input deck. 
TITLE 
A description of this coupling definition. 
SLAVE 
Slave  set  ID  defining  a  part,  part  set  ID  of  the  Lagrangian  beam 
structure .
VARIABLE   
MASTER 
DESCRIPTION
Master  set  ID  defining  a  part  or  part  set  ID  of  the  Lagrangian 
solid elements or thick shell elements . 
SSTYP 
Slave set type of “SLAVE”: 
EQ.0: part set ID (PSID). 
EQ.1: part ID (PID). 
MSTYP 
Master set type of “MASTER”: 
EQ.0: part set ID (PSID). 
EQ.1: part ID (PID). 
NCOUP 
Number of coupling points generated in one beam element.  If set
to 0, coupling only happens at beam nodes.  Otherwise, coupling
is done at both the beam nodes and those automatically generated 
coupling points. 
CDIR 
Coupling direction. 
EQ.0: default, constraint applied along all directions. 
EQ.1: Constraint  only  applied  along  normal  directions;  along
the beam axial direction there is no constraint.  
START 
Start time for coupling. 
END 
End time for coupling. 
AXFOR 
ID of a user defined function describes coupling force versus slip
along beam axial direction. 
GE.0: 
EQ.-n: 
OFF 
n is the function ID in *DEFINE_FUNCTION 
EQ.n > 1000: 
n  is  the  debonding  law  id  “lawid”  in  user 
defined subroutine rebar_bondslip_get_force(). 
Example: 
1.    The  example  below  shows  how  to  define  a  function  and  use  it  to  prescribe  the 
debonding  process.    User  can  define  his  own  function  based  on  different  debonding 
theories. 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...
.8
*CONSTRAINED_BEAM_IN_SOLID 
$#      slave        master          sstyp          mstyp          ctype          empty          nquad      
idir 
         2         1         1         1         0                     2         
1 
$#   start       end               axfor 
     0.000     0.000                 -10 
*DEFINE_FUNCTION 
        10 
float force(float slip,float leng) 
{ 
float force,pi,d,area,shear,pf; 
pi = 3.1415926; 
d = 0.175; 
area = pi*d*leng; 
pf = 1.0; 
if (slip < 0.25) { 
shear = slip*pf; 
} else { 
shear = 0.25*pf; 
} 
force = shear*area; 
return force; 
} 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...
.8 
2.  The example below shows how to define a user subroutine and use it to prescribe the 
debonding process.  
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...
.8 
*CONSTRAINED_BEAM_IN_SOLID 
$#      slave        master          sstyp          mstyp          ctype          empty          nquad      
idir 
         2         1         1         1         0                    2         
1 
$#   start       end               axfor 
     0.000     0.000                1001 
*CONSTRAINED_BEAM_IN_SOLID 
$#      slave        master          sstyp          mstyp          ctype          empty          nquad      
idir 
         3         1         1         1         0                     2         
1 
$#   start       end               axfor 
     0.000     0.000                1002 
*USER_LOADING 
$        parm1          parm2          parm3          parm4          parm5          parm6          parm7     
parm8 
       1.0       6.0 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...
.8 
And the user debonding law subroutine: 
      subroutine rebar_bondslip_get_force(slip,dl,force,hsv,
.  userparm,lawid) 
      real hsv 
      dimension hsv(12),cm(8),userparm(*) 
c 
c in this subroutine user defines debonding properties and 
c call his own debonding subroutine to get force 
      cm(1)=userparm(1) 
      cm(2)=userparm(2) 
      cm(3)=2.4*(cm(2)/5.0)**0.75 
      cm(8)=0. 
c 
      pi = 3.1415926 
      d = 0.175 
      area = pi*0.25*d*d*dl 
      pf = 1.0 
c 
      if (lawid.eq.1001) then 
        if (slip.lt.0.25) then 
          shear = slip*pf 
        else 
          shear = 0.25*pf 
        endif 
        force = sign(1.0,slip)*shear*area 
      elseif (lawid.eq.1002) then 
        if (slip.lt.0.125) then 
          shear = slip*pf 
        else 
          shear = 0.125*pf 
        endif 
      endif 
      return 
      end
*CONSTRAINED_BUTT_WELD 
Purpose:    Define  a  line  of  coincident  nodes  that  represent  a  structural  butt  weld 
between two parts defined by shell elements.  Failure is based on nodal plastic strain for 
ductile failure and stress resultants for brittle failure.  This input is much simpler than 
the  alternative  approach  for  defining  butt  welds,  see  *CONSTRAINED_GENERAL-
IZED_WELD_BUTT.    The  local  coordinate  system,  the  effective  length,  and  thickness 
for  each  pair  of  butt  welded  nodes  are  determined  automatically  in  the  definition 
below.  In the GENERALIZED option these quantities must be defined in the input. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SNSID 
MNSID 
EPPF 
SIGF 
BETA 
Type 
I 
I 
F 
F 
F 
Default 
none 
none 
0. 
1.e+16 
1.0 
Remarks 
1, 2 
3, 4 
3 
3 
  VARIABLE   
DESCRIPTION
SNSID 
Slave node set ID, see *SET_NODE_OPTION. 
MNSID 
Master node set ID, see *SET_NODE_OPTION. 
EPPF 
SIGF 
Plastic strain at failure 
𝜎𝑓 , stress at failure for brittle failure. 
BETA 
𝛽, failure parameter for brittle failure.
Remarks: 
1.  Nodes  in  the  master  and  slave  sets  must  be  given  in  the  order  they  appear  as 
one moves along the edge of the surface.  An equal number of coincident nodes 
must be defined in each set.  In a line weld the first and last node in a string of 
nodes can be repeated in the two sets.  If the first and last pair of nodal points 
are identical, a circular or closed loop butt weld is assumed.   See Figure 10-1, 
where the line butt weld and closed loop weld are illustrated.
local y-axis
Length of
butt weld
Repeated nodal point
may start or end a butt
weld line. This beginning
or ending nodal point
must exist in both and
slave and master definitions
Two coincident butt welded
nodal points.
Repeated nodal point
pair must start and end
circular butt weld. Any
nodal pair in the circle
can be used.
Figure 10-1.  Definition of butt welds are shown above.  The butt weld can be
represented by a line of nodal points or by a closed loop 
2.  Butt welds may not cross.  For complicated welds, this option can be combined 
with  the  input  in  *CONSTRAINED_GENERALIZED_WELD_BUTT  to  handle 
the case where crossing occurs.  Nodes in a butt weld must not be members of 
rigid bodies.
3. 
If  the  average  volume-weighted  effective  plastic  strain  in  the  shell  elements 
adjacent  to  a  node  exceeds  the  specified  plastic  strain  at  failure,  the  node  is 
released.  Brittle failure of the butt welds occurs when: 
𝛽√𝜎𝑛
2 + 3(𝜏𝑛
2 + 𝜏𝑡
2) ≥ 𝜎𝑓  
where, 
𝜎𝑛 = normal stress (local x) 
𝜏𝑛 = shear stress in direction of weld (local y) 
𝜏𝑡 = shear stress normal to weld (local z) 
𝜎𝑓 = failure stress 
𝛽 = failure parameter 
The  component  σn  is  nonzero  for  tensile  values  only.    The  nodes  defining  the 
slave  and  master  sides  of  the  butt  weld  must  coincide.    The  local  z-axis  at  a 
master node is normal to the master side plane of the butt weld at the node, and 
the  local  y-axis  is  taken  as  the  vector  in  the  direction  of  a  line  connecting  the 
mid-points  of  the  line  segments  lying  on  either  side  of  the  master  node.    The 
normal  vector  is  found  by  summing  the  unit  normal  vectors  of  all  shell  ele-
ments  on  the  master  side  sharing  the  butt  welded  node.    The  direction  of  the 
normal vector at the node is chosen so that the x-local vector points towards the 
elements  on  the  slave  side  in  order  to  identify  tensile  versus  compressive 
stresses.  The thickness of the butt weld and length of the butt weld are needed 
to compute the stress values.  The thickness is based on the average thickness of 
the shell elements that share the butt welded nodal pair, and the chosen length 
of the butt weld is shown in Figure 10-1. 
4.  Butt welds may be used to simulate the effect of failure along a predetermined 
line, such as a seam or structural joint.  When the failure criterion is reached at a 
nodal pair, the nodes begin to separate.  As this effect propagates, the weld will 
appear to “unzip,” thus simulating failure of the connection.
*CONSTRAINED_COORDINATE_{OPTION} 
To define constraints based on position coordinates the following options are available: 
<BLANK> 
LOCAL 
Purpose:    The  keyword  is  developed  to  allow  the  definition  of  constraints  in  position 
coordinates in springback simulation.  With the frequent application of adaptive mesh 
in stamping simulation, nodes needed for springback constraints are often unavailable 
until  the  last  process  simulation  before  springback  is  complete.    On  the  other  hand,  if 
the  nodes  are  available,  their  positions  may  not  be  exactly  on  the  desired  locations 
required for springback constraints.  With this new keyword, the springback simulation 
is  no  longer  dependent  on  the  previous  process  simulation  results  and  the  exact 
springback constraint locations can be specified. 
  Card 1 
Variable 
1 
ID 
2 
3 
PID 
IDIR 
Type 
I 
I 
I 
4 
X1 
F 
5 
Y1 
F 
6 
Z1 
F 
Default 
none 
none 
none 
0.0 
0.0 
0.0 
8 
7 
CID 
I 
0 
  VARIABLE   
DESCRIPTION
ID 
PID 
IDIR 
Identification number of a constraint. 
Part ID of the part to be constrained. 
Applicable degrees-of-freedom being constrained: 
EQ.1:  x translational degree-of-freedom, 
EQ.2:  y translational degree-of-freedom, 
EQ.3:  z translational degree-of-freedom. 
X1, Y1, Z1 
X, Y, Z coordinates of the location being constrained. 
CID 
Local coordinate system ID.
Figure  10-2.    Constrained  locations  of  a  trim  panel  (NUMISHEET  2005  cross
member). 
General remarks: 
The identification number of a constraint must be unique;  in particular, the IDs must be 
unique  even  for  two  constraints  involving  the  same  X,  Y,  Z  coordinates  but  different 
degrees of freedom.  When the LOCAL option is invoked, a local coordinate system ID, 
as  defined  with  *DEFINE_COORDINATE_{OPTION}  keyword,  should  be  provided  in 
the CID field. 
Defining  constraints  using  coordinates  can  now  be  done  in  Springback  process  of  LS-
PrePost4.0 eZSetup for metal forming application, using the Pick location button (http://-
ftp.lstc.com/anonymous/outgoing/lsprepost/4.0/metalforming/). 
Application example: 
An example of using the keyword is listed below.  A part with PID 18 is constrained in 
6 locations in a local coordinate system ID 9, defined by the keyword *DEFINE_COOR-
DINATE_SYSTEM.  Constrained DOFs are indicated by IDIR. 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*CONSTRAINED_COORDINATE 
$       ID      IDPT      IDIR         x         y         z       CID 
         1        18         2  -555.128      86.6   1072.29         9 
         2        18         3  -555.128      86.6   1072.29         9 
         3        18         3  -580.334    -62.15   1068.32         9 
         4        18         1   568.881   81.2945   1033.72         9 
         5        18         2   568.881   81.2945   1033.72         9 
         6        18         3   568.881   81.2945   1033.74         9
)
(
-
)
(
-
150
100
50
-50
-100
SPC Force @ Nodes
                         A
                         B
                         C
                         D
                         E
                         F
                         G
                         H
                          I
                          J
0.2
0.4
0.6
0.8
Time (Sec.)
Figure 10-3.  SPC Z-forces at 10 nodes. 
140
120
100
80
60
40
20
SPC Force @ Nodes
                        Sum SPC force 10 nodes
0.2
0.4
0.6
0.8
Time (Sec.)
Figure 10-4.  SPC Z-force summation of the 10 nodes 
*DEFINE_COORDINATE_SYSTEM 
$      CID        X0        Y0        Z0        XL        YL        ZL 
         9       0.0       0.0       0.0       0.0      10.0       0.0 
$       XP        YP        ZP 
      10.0      10.0       0.0 
It  is  possible  to  output  SPC  forces  on  the  coordinates  constrained.    For  each  position 
coordinate  set,  an  extra  node  will  be  generated  and  SPC  forces  are  calculated  and 
output  to  SPCFORC  file.    The  frequency  of  the  output  is  specified  with  the  keyword 
*DATABASE_SPCFORC.  Shown in the Figure 10-2 are the Z-constrained locations on 
the  trimmed  panel  (half  with  symmetric  conditions  at  the  smaller  end)  of  the 
NUMISHEET 2005 cross member.  SPC forces in Z direction of these 10 locations were 
recovered  after  a  multi-steps  static  implicit  springback  with  this  over-constrained 
boundary condition, Figure 10-3.  The summation of these Z-forces is shown in Figure 
10-4  and  it  approaches  to  zero  as  the  residual  stresses  are  balanced  out  by  the 
springback shape, absent of gravity.
Revision information: 
This feature is now available in LS-DYNA R5 Revision 52619 or later releases.  The SPC 
output feature is available in LS-DYNA Revision 62560 and later releases, both in SMP 
and MPP.
*CONSTRAINED_EULER_IN_EULER 
Purpose:    This  command  defines  the  coupling  interaction  between  EULERIAN 
materials in two overlapping, geometrically similar, multi-material Eulerian mesh sets.  
The  command  allows  a  frictionless  “contact”  between  two  or  more  different  Eulerian 
materials. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PSIDSLV  PSIDMST 
PFAC 
Type 
Default 
I 
0 
I 
0 
F 
0.1 
  VARIABLE   
DESCRIPTION
PSIDSLV 
Part set ID of the 1st ALE or Eulerian set of mesh(es) (slave). 
PSIDMST 
Part set ID of the 2nd ALE or Eulerian set of mesh(es) (master). 
PFAC 
A  penalty  factor  for  the  coupling  interaction  between  the  two
PSIDs. 
Remarks: 
1.  The  2  meshes  must  be  of  Eulerian  formulation  (the  meshes  are  fixed  in  space, 
not  moving).    Consider  2  overlapping  Eulerian  meshes.    Each  Eulerian  mesh 
contains 2 physical materials, say a vacuum and a metal.  This card provides a 
frictionless “contact” or interaction between the 2 metals, each resides in a dif-
ferent  Eulerian  mesh  system.    Due  to  its  restrictive  nature,  this  option  is  cur-
rently only an experimental feature. 
2.  Contact  pressure  is  built  up  in  two  overlapping  Eulerian  elements  if  their 
combined material fill fraction exceeds 1.0 (penalty formulation). 
3.  This  feature  needs  to  be  combined  with  *MAT_VACUUM  (element  formula-
tion 11). 
Example: 
Consider an ALE/Eulerian multi-material model (ELFORM = 11) consisting of:
PID 1 = *MAT_NULL (material 1) 
PID 2 = *MAT_VACUUM ⇒ PID 1 is merged at its boundary to PID 2. 
PID 3 = *MAT_NULL (material 3) 
PID 4 = *MAT_VACUUM ⇒ PID 3 is merged at its boundary to PID 4. 
The mesh set containing PID 1 & 2 intersects or overlaps with the mesh set containing 
PID 3 & 4.  PID 1 is given an initial velocity in the positive x direction.  This will cause 
material  1  to  contact  material  3  (note  that  materials  2  &  4  are  void).    The  interaction 
between  materials  1  &  3  is  possible  by  defining  this  coupling  command.    In  this  case 
material 1 can flow within the mesh region of PID 1 & 2 only, and material 3 can flow 
within the mesh region of PID 3 & 4 only. 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 
*ALE_MULTI-MATERIAL_GROUP 
$      SID   SIDYTPE  
         1         1 
         2         1 
         3         1 
         4         1 
*CONSTRAINED_EULER_IN_EULER 
$    PSID1     PSID2     PENAL 
        11        12       0.1 
*SET_PART_LIST 
        11 
         1         2 
*SET_PART_LIST 
        12 
         3         4 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8
*CONSTRAINED_EXTRA_NODES_OPTION 
Available options include: 
NODE 
SET 
Purpose:  Define extra nodes for rigid body. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
NID/NSID 
IFLAG 
Type 
I 
I 
Default 
none 
none 
I 
0 
  VARIABLE   
PID 
DESCRIPTION
Part  ID  of  rigid  body  to  which  the  nodes  will  be  added,  see
*PART. 
NID / NSID 
Node (keyword option: NODE) or node set ID (keyword option:
SET), see *SET_NODE, of added nodes. 
This flag is meaningful if and only if the inertia properties of the
Part ID are defined in PART_INERTIA.  If set to unity, the center-
of-gravity,  the  translational  mass,  and  the  inertia  matrix  of  the
PID  will  be  updated  to  reflect  the  merged  nodal  masses  of  the
node  or  node  set.      If  IFLAG  is  defaulted  to  zero,  the  merged
nodes  will  not  affect  the  properties  defined  in  PART_INERTIA 
since  it  is  assumed  the  properties  already  account  for  merged
nodes. 
IFLAG 
Remarks: 
Extra nodes for rigid bodies may be placed anywhere, even outside the body, and they 
are assumed to be part of the rigid body.  They have many uses including: 
1.  The  definition  of  draw  beads  in  metal  forming  applications  by  listing  nodes 
along the draw bead. 
2.  Placing nodes where joints will be attached between rigid bodies.
3.  Defining a node where point loads are to be applied or where springs may be 
attached. 
4.  Defining a lumped mass at a particular location. 
The coordinates of the extra nodes are updated according to the rigid body motion. 
Examples: 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *CONSTRAINED_EXTRA_NODES_NODE 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Rigidly attach nodes 285 and 4576 to part 14.  (Part 14 MUST be a rigid body.) 
$ 
*CONSTRAINED_EXTRA_NODES_NODE 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      pid       nid 
        14       285 
        14      4576 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *CONSTRAINED_EXTRA_NODES_SET 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Rigidly attach all nodes in set 4 to part 17.  (Part 17 MUST be a rigid body.) 
$ 
$  In this example, four nodes from a deformable body are attached 
$  to rigid body 17 as a means of joining the two parts. 
$ 
*CONSTRAINED_EXTRA_NODES_SET 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      pid      nsid 
        17         4 
$ 
$ 
*SET_NODE_LIST 
$      sid 
         4 
$     nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
       665       778       896       827 
$ 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$
*CONSTRAINED_GENERALIZED_WELD_OPTION_{OPTION} 
Available options include: 
SPOT 
FILLET 
BUTT 
CROSS_FILLET 
COMBINED 
To define an ID for the weld use the option: 
ID 
Purpose:    Define  spot,  fillet,  butt,  and  other  types  of  welds.    Coincident  nodes  are 
permitted if the local coordinate ID is defined.  For the spot weld a local coordinate ID 
is not required if the nodes are offset.  Failures can include both the plastic and brittle 
failures.    These  can  be  used  either  independently  or  together.    Failure  occurs  when 
either  criteria  is  met.    The  welds  may  undergo  large  rotations  since  the  equations  of 
rigid body mechanics are used to update their motion.  Weld constraints between solid 
element nodes are not supported. 
ID Card.  Additional card for ID keyword option. 
  ID Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
WID 
Type 
Default 
I
Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSID 
CID 
FILTER  WINDOW
NPR 
NPRT 
Type 
I 
I 
I 
E 
I 
I 
Default 
none 
none 
  VARIABLE   
DESCRIPTION
WID 
NSID 
CID 
FILTER 
WINDOW 
Optional weld ID. 
Nodal set ID, see *SET_NODE_OPTION. 
Coordinate system ID for output of spot weld data to SWFORC in
local system, see *DEFINE_COORDINATE_OPTION.  CID is not 
required for spot welds if the nodes are not coincident. 
Number  of  force  vectors  saved  for  filtering.    This  option  can
eliminate  spurious  failures  due  to  numerical  force  spikes;
however,  memory  requirements  are  significant  since  6  force
components are stored with each vector. 
LE.1:  no filtering 
GE.2:  simple  average  of  force  components  divided  by  FILTER 
or the maximum number of force vectors that are stored
for the time window option below. 
Time window for filtering.  This option requires the specification
of  the  maximum  number  of  steps  which  can  occur  within  the 
filtering time window.  If the time step decreases too far, then the
filtering  time  window  will  be  ignored  and  the  simple  average  is
used. 
EQ.0: time window is not used 
NPR 
Number of individual nodal pairs in the cross fillet or combined
general weld.
VARIABLE   
DESCRIPTION
NPRT 
Print option in file rbdout. 
EQ.0: default  from  the  control  card,  *CONTROL_OUTPUT,  is 
used, see variable name IPRTF. 
EQ.1: data is printed 
EQ.2: data is not printed 
Spot Weld Card.  Additional Card required SPOT keyword option. 
  Card 2 
1 
2 
Variable 
TFAIL 
EPSF 
Type 
F 
F 
3 
SN 
F 
4 
SS 
F 
5 
N 
F 
6 
M 
F 
7 
8 
  VARIABLE   
DESCRIPTION
TFAIL 
Failure time for constraint set, tf .  (default = 1.E+20) 
Effective plastic strain at failure, 𝜖fail
𝑝  defines ductile failure. 
Sn,  normal  force  at  failure,  only  for  the  brittle  failure  of  spot
welds. 
Ss, shear force at failure, only for the brittle failure of spot welds. 
n,  exponent  for  normal  force,  only  for  the  brittle  failure  of  spot
welds. 
m,  exponent  for  shear  force,  only  for  the  brittle  failure  of  spot 
welds. 
EPSF 
SN 
SS 
N 
M 
Remarks: 
Spot weld failure due to plastic straining occurs when the effective nodal plastic strain 
𝑝 .  This option can model the tearing out of a spot weld from 
exceeds the input value, 𝜀fail
the sheet metal since the plasticity is in the material that surrounds the spot weld, not 
the spot weld itself.  A least squares algorithm is used to generate the nodal values of 
plastic strains at the nodes from the element integration point values.  The plastic strain 
is integrated through the element and the average value is projected to the nodes via a
node 3
node 2
node 1
node 2
node 1
2 NODE SPOTWELD
xx
node N
node N - 1
N NODE SPOTWELD
node 2
node 1
Figure 10-5.  Nodal ordering and orientation of the local coordinate system is
important for determining spotweld failure. 
least  square  fit.    This  option  should  only  be  used  for  the  material  models  related  to 
metallic plasticity and can result in slightly increased run times. 
Brittle failure of the spot welds occurs when: 
[
max(𝑓𝑛, 0)
𝑆𝑛
]
+ [
∣𝑓𝑠∣
𝑆𝑠
]
≥ 1 
where fn and fs are the normal and shear interface force.  Component fn contributes for 
tensile values only.  When the failure time, tf, is reached the nodal rigid body becomes 
inactive and the constrained nodes may move freely.  In Figure 10-5 the ordering of the 
nodes is shown for the 2 node and 3 node spot welds.  This order is with respect to the 
local  coordinate  system  where  the  local  z-axis  determines  the  tensile  direction.    The
nodes  in  the  spot  weld  may  coincide.    The  failure  of  the  3  node  spot  weld  may  occur 
gradually with first one node failing and later the second node may fail.  For n noded 
spot  welds  the  failure  is  progressive  starting  with  the  outer  nodes  (1  and  n)  and  then 
moving  inward  to  nodes  2  and  n -  1.    Progressive  failure  is  necessary  to  preclude 
failures that would create new rigid bodies. 
Fillet Weld Card.  Additional Card required for the FILLET keyword option. 
  Card 2 
1 
2 
3 
4 
Variable 
TFAIL 
EPSF 
SIGF 
BETA 
Type 
F 
F 
F 
F 
5 
L 
F 
6 
W 
F 
7 
A 
F 
8 
ALPHA 
F 
  VARIABLE   
DESCRIPTION
TFAIL 
Failure time for constraint set, tf   (default = 1.E+20). 
EPSF 
SIGF 
Effective plastic strain at failure, 𝜖fail
𝑝  defines ductile failure. 
𝜎𝑓 , stress at failure for brittle failure. 
BETA 
𝛽, failure parameter for brittle failure. 
L 
W 
A 
L, length of fillet weld . 
w, separation of parallel fillet welds . 
a, fillet weld throat dimension . 
ALPHA 
𝛼, weld angle  in degrees. 
Remarks: 
Ductile  fillet  weld  failure,  due  to  plastic  straining,  is  treated  identically  to  spot  weld 
failure.    Brittle  failure  occurs  when  the  following  weld  stress  condition  is  met  on  the 
narrowest fillet weld cross section (across the throat): 
𝛽√𝜎𝑛
2 + 3(𝜏𝑛
2 + 𝜏𝑡
2) ≥ 𝜎𝑓  
Where 
𝜎𝑛 = normal stress 
𝜏𝑛 = shear stress in local z-x plane 
𝜏𝑡 = 𝑠hear stress in local-y direction
2 Node Fillet Weld
local coordinate
system
3 Node Fillet Weld
Figure 10-6.  Nodal ordering and orientation of the local coordinate system is 
shown for fillet weld failure.  The angle is defined in degrees. 
𝜎𝑓 = failure stress 
𝛽 = failure parameter 
The  component  𝜎𝑛  is  nonzero  for  tensile  values  only.    When  the  failure  time,  𝑡𝑓   ,  is 
reached  the  nodal  rigid  body  becomes  inactive  and  the  constrained  nodes  may  move 
freely.  In Figure 10-6 the ordering of the nodes is shown for the 2 node and 3 node fillet 
welds.  This order is with respect to the local coordinate system where the local z axis 
determines the tensile direction.  The initial orientation of the local coordinate system is 
defined  by  CID.    If  CID = 0  then  the  global  coordinate  system  is  used.    The  local 
coordinate  system  is  updated  according  to  the  rotation  of  the  rigid  body  representing 
the weld.  The failure of the 3 node fillet weld may occur gradually with first one node 
failing and later the second node may fail.
LL
11
22
11
22
22
11
22
11
22
11
22
11
22
11
22
2 tied nodes that can
be coincident
Figure 10-7.  Orientation of the local coordinate system and nodal ordering is
shown for butt weld failure. 
Butt Weld Card.  Additional Card required for the BUTT keyword option. 
  Card 2 
1 
2 
3 
4 
Variable 
TFAIL 
EPSF 
SIGY 
BETA 
Type 
F 
F 
F 
F 
5 
L 
F 
6 
D 
F 
8 
  VARIABLE   
DESCRIPTION
TFAIL 
Failure time for constraint set, tf .  (default = 1.E+20) 
EPSF 
SIGY 
Effective plastic strain at failure, 𝜖fail
𝑝  defines ductile failure. 
𝜎𝑓 , stress at failure for brittle failure. 
BETA 
𝛽, failure parameter for brittle failure. 
L, length of butt weld . 
d, thickness of butt weld . 
L 
D 
Remarks: 
Ductile  butt  weld  failure,  due  to  plastic  straining,  is  treated  identically  to  spot  weld 
failure.  Brittle failure of the butt welds occurs when: 
𝛽√𝜎𝑛
2 + 3(𝜏𝑛
2 + 𝜏𝑡
2) ≥ 𝜎𝑓  
where
𝜎𝑛 = normal stress 
𝜏𝑛 = shear stress in direction of weld (local y) 
𝜏𝑡 = shear stress normal to weld (local z) 
𝜎𝑓 = failure stress 
𝛽 = failure parameter 
The  component  σn  is  nonzero  for  tensile  values  only.    When  the  failure  time,  tf  ,  is 
reached  the  nodal  rigid  body  becomes  inactive  and  the  constrained  nodes  may  move 
freely.  The nodes in the butt weld may coincide. 
Example: 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *CONSTRAINED_GENERALIZED_WELD_BUTT 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Weld two plates that butt up against each other at three nodal pair 
$  locations.  The nodal pairs are 32-33, 34-35 and 36-37. 
$ 
$  This requires 3 separate *CONSTRAINED_GENERALIZED_WELD_BUTT definitions, 
$  one for each nodal pair.  Each weld is to have a length (L) = 10, 
$  thickness (D) = 2, and a transverse length (Lt) = 1. 
$ 
$  Failure is defined two ways: 
$    Ductile failure if effective plastic strain exceeds 0.3 
$    Brittle failure if the stress failure criteria exceeds 0.25 
$       - scale the brittle failure criteria by beta = 0.9. 
$    Note: beta > 1 weakens weld          beta < 1 strengthens weld 
$ 
*CONSTRAINED_GENERALIZED_WELD_BUTT 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$     nsid       cid 
        21 
$    tfail      epsf      sigy      beta         L         D        Lt 
                 0.3     0.250       0.9      10.0       2.0       1.0 
$ 
$ 
*CONSTRAINED_GENERALIZED_WELD_BUTT 
$     nsid       cid 
        23 
$    tfail      epsf      sigy      beta         L         D        Lt 
                 0.3     0.250       0.9      10.0       2.0       1.0 
$ 
$ 
*CONSTRAINED_GENERALIZED_WELD_BUTT 
$     nsid       cid 
        25 
$    tfail      epsf      sigy      beta         L         D        Lt 
                 0.3     0.250       0.9      10.0       2.0       1.0 
$ 
$ 
*SET_NODE_LIST 
$      sid 
        21
$     nid1      nid2 
        32        33 
*SET_NODE_LIST 
        23 
        34        35 
*SET_NODE_LIST 
        25 
        36        37 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
Cross Fillet Weld Card.  Additional Card for the CROSS_FILLET keyword option. 
  Card 2 
1 
2 
3 
4 
Variable 
TFAIL 
EPSF 
SIGY 
BETA 
Type 
F 
F 
F 
F 
5 
L 
F 
6 
W 
F 
7 
A 
F 
8 
ALPHA 
F 
Nodal  Pair  Cards.    Read  NPR  additional  cards  for  the  CROSS_FILLET  keyword 
option. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NODEA 
NODEB 
NCID 
Type 
I 
I 
I 
  VARIABLE   
DESCRIPTION
TFAIL 
Failure time for constraint set, tf .  (default = 1.E+20) 
EPSF 
SIGY 
Effective plastic strain at failure, 𝜖fail
𝑝  defines ductile failure. 
𝜎𝑓 , stress at failure for brittle failure. 
BETA 
𝛽, failure parameter for brittle failure. 
L 
W 
A 
L, length of fillet weld . 
w, separation of parallel fillet welds . 
a, throat dimension of fillet weld . 
ALPHA 
𝛼, weld angle  in degrees.
y2
(a)
z1
y1
x1
z2
x2
(c)
(b)
y3
x3
z3
(d)
Figure  10-8.    A  simple  cross  fillet  weld  illustrates  the  required  input.    Here
NPR = 3 with nodal pairs (A = 2, B = 1), (A = 3, B = 1), and (A = 3, B = 2).  The
local coordinate axes are shown.  These axes are fixed in the rigid body and are
referenced  to  the  local  rigid  body  coordinate  system  which  tracks  the  rigid
body rotation. 
  VARIABLE   
NODEA 
DESCRIPTION
Node ID, A, in weld pair (CROSS or COMBINED option only). 
See Figure 10-8.
VARIABLE   
DESCRIPTION
NODEB 
Node ID, B, in weld pair (CROSS or COMBINED option only). 
NCID 
Local coordinate system ID (CROSS or COMBINED option only).
Combined Weld Cards: 
Additional  cards  for  the  COMBINED  keyword  option.    Read  in  NPR  pairs  of  Cards  2 
and 3 for a total of 2 × NPR cards. 
  Card 2 
1 
2 
3 
4 
Variable 
TFAIL 
EPSF 
SIGY 
BETA 
Type 
F 
  Card 3 
1 
F 
2 
F 
3 
F 
4 
Variable 
NODEA 
NODEB 
NCID 
WTYP 
Type 
I 
I 
I 
I 
5 
L 
F 
5 
6 
W 
F 
6 
7 
A 
F 
7 
8 
ALPHA 
F 
8 
  VARIABLE   
DESCRIPTION
TFAIL 
Failure time for constraint set, tf .  (default = 1.E+20) 
EPSF 
SIGY 
Effective plastic strain at failure, 𝜖fail
𝑝  defines ductile failure. 
𝜎𝑓 , stress at failure for brittle failure. 
BETA 
𝛽, failure parameter for brittle failure. 
L 
W 
A 
L, length of fillet/butt weld . 
w, width of flange . 
a, width of fillet weld . 
ALPHA 
𝛼, weld angle  in degrees.
3 node
Fillet
Butt Weld
Figure 10-9.  A combined weld is a mixture of fillet and butt welds. 
  VARIABLE   
DESCRIPTION
NODEA 
Node ID, A, in weld pair (CROSS or COMBINED option only). 
NODEB 
Node ID, B, in weld pair (CROSS or COMBINED option only). 
NCID 
Local coordinate system ID (CROSS or COMBINED option only).
WTYPE 
Weld pair type (GENERAL option only).  See Figure 10-9. 
EQ.0: fillet weld 
EQ.1: butt weld
*CONSTRAINED_GLOBAL 
7 
8 
Purpose:  Define a global boundary constraint plane. 
  Card 1 
Variable 
Type 
Default 
1 
TC 
I 
0 
2 
RC 
I 
0 
3 
DIR 
I 
0 
4 
X 
F 
0 
5 
Y 
F 
0 
6 
Z 
F 
0 
  VARIABLE   
DESCRIPTION
TC 
Translational Constraint: 
EQ.1: constrained x translation, 
EQ.2: constrained y translation, 
EQ.3: constrained z translation, 
EQ.4: constrained x and y translations, 
EQ.5: constrained y and z translations, 
EQ.6: constrained x and z translations, 
EQ.7: constrained x, y, and z translations, 
RC 
Rotational Constraint: 
EQ.1: constrained x-rotation, 
EQ.2: constrained y-rotation, 
EQ.3: constrained z-rotation, 
EQ.4: constrained x and y rotations, 
EQ.5: constrained y and z rotations, 
EQ.6: constrained z and x rotations, 
EQ.7: constrained x, y, and z rotations.
VARIABLE   
DESCRIPTION
DIR 
Direction of normal for constraint plane. 
EQ.1: global x, 
EQ.2: global y, 
EQ.3: global z. 
X 
Y 
Z 
Global x-coordinate of a point on the constraint plane. 
Global y-coordinate of a point on the constraint plane. 
Global z-coordinate of a point on the constraint plane. 
Remarks: 
Nodes within a mesh-size-dependent tolerance are constrained on a global plane.  This 
option  is  recommended  for  use  with  r-method  adaptive  remeshing  where  nodal 
constraints  are  lost  during  the  remeshing  phase.    See  *CONSTRAINED_LOCAL  for 
specifying constraints to nodes lying on a local plane.
*CONSTRAINED_INTERPOLATION_{OPTION} 
Available options include: 
<BLANK> 
LOCAL 
Purpose:  Define an interpolation constraint.  With this constraint type, the motion of a 
single dependent node is interpolated from the motion of a set of independent nodes. 
This option is useful for the redistribution of a load applied to the dependent node by 
the  surrounding  independent  nodes.    This  load  may  be  a  translational  force  or  a 
rotational moment.  This keyword is typically used to model shell-brick and beam-brick 
interfaces. 
The  mass  and  rotary  inertia  of  the  dependent  nodal  point  is  also  redistributed.    This 
constraint is applied in the global coordinate system unless the option LOCAL is active.  
One  *CONSTRAINED_INTERPOLATION  card  is  required  for  each  constraint  definition.  
The input list of independent nodes is terminated when the next "*" card is found.  In 
explicit  calculations  the  independent  nodes  cannot  be  dependent  nodes  in  other 
constraints such as nodal rigid bodies; however, implicit calculations are not bound by 
this limitation. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ICID 
DNID 
DDOF 
CIDD 
ITYP 
Type 
Default 
I 
0 
I 
I 
I 
0 
123456 optional
I
Independent Node Card Sets: 
If LOCAL option is not set, for each independent node include the following card; if the 
LOCAL  keyword  option  is  set,  include  only  the  following  pair  of  cards.    This  input  is 
terminated at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
INID 
IDOF 
TWGHTX  TWGHTY  TWGHTZ  RWGHTX  RWGHTY  RWGHTZ 
Type 
I 
I 
F 
F 
F 
F 
F 
F 
Default 
0 
123456 
1.0 
TWGHTX  TWGHTX  TWGHTX  TWGHTX  TWGHTX 
Local Coordinate Card.  Additional card for the LOCAL keyword option to be paired 
with card 2. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CIDI 
Type 
Default 
I 
0 
  VARIABLE   
DESCRIPTION
ICID 
DNID 
DDOF 
Interpolation constraint ID. 
Dependent node ID.  This node should not be a member of a rigid
body, or elsewhere constrained in the input. 
Dependent degrees-of-freedom.  The list of dependent degrees-of-
freedom  consists  of  a  number  with  up  to  six  digits,  with  each
digit  representing  a  degree  of  freedom.    For  example,  the  value
1356 indicates that degrees of freedom 1, 3, 5, and 6 are controlled 
by the constraint.  The default is 123456.  Digit: degree of freedom
ID's: 
EQ.1: x 
EQ.2: y
VARIABLE   
DESCRIPTION
EQ.3: z 
EQ.4: rotation about x axis 
EQ.5: rotation about y axis 
EQ.6: rotation about z axis 
CIDD 
Local  coordinate  system  ID  if  LOCAL  option  is  active.    If  blank
the global coordinate system is assumed. 
ITYP 
Specifies the meaning of INID. 
EQ.0: INID is a node ID 
EQ.1: INID is a node set ID 
Independent node ID or node set ID. 
Independent  degrees-of-freedom  using  the  same  form  as  for  the 
dependent degrees-of-freedom, DDOF, above. 
Weighting  factor  for  node  INID  with  active  degrees-of-freedom 
IDOF.    This  weight  scales  the  x-translational  component.    It  is 
normally sufficient to define only TWGHTX even if its degree-of-
freedom  is  inactive  since  the  other  factors  are  set  equal  to  this
input value as the default.  There is no requirement on the values
that  are  chosen  as  the  weighting  factors,  i.e.,  that  they  sum  to
unity.  The default value for the weighting factor is unity. 
Weighting  factor  for  node  INID  with  active  degrees-of-freedom 
IDOF.  This weight scales the y-translational component.    
Weighting  factor  for  node  INID  with  active  degrees-of-freedom 
IDOF.  This weight scales the z-translational component. 
Weighting  factor  for  node  INID  with  active  degrees-of-freedom 
IDOF.  This weight scales the x-rotational component. 
Weighting  factor  for  node  INID  with  active  degrees-of-freedom 
IDOF.  This weight scales the y-rotational component. 
Weighting  factor  for  node  INID  with  active  degrees-of-freedom 
IDOF.  This weight scales the z-rotational component. 
INID 
IDOF 
TWGHTX 
TWGHTY 
TWGHTZ 
RWGHTX 
RWGHTY 
RWGHTZ 
CIDI 
Local  coordinate  system  ID  if  LOCAL  option  is  active.    If  blank
the global coordinate system is assumed.
21
22
11
45
44
33
43
Figure 10-10.  Illustration of Example 1. 
Example 1: 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *CONSTRAINED_INTERPOLATION  (Beam to solid coupling) 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Tie a beam element to a solid element. 
$ 
$  The node of the beam to be tied does not share a common node with the solids. 
$  If the beam node is shared, for example, then set ddof=456. 
$ 
*CONSTRAINED_INTERPOLATION 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$     icid      dnid      ddof 
         1        45    123456 
$     inid      idof    twghtx    twghty    twghtz    rwghtx    rwghty    rwghtz 
        22       123 
        44       123 
        43       123 
$ 
*......... 
$
180
179
178
177
100
99
98
97
96
Figure 10-11.  Illustration of Example 2. 
Example 2: 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *CONSTRAINED_INTERPOLATION  (Load redistribution) 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Moment about normal axis of node 100 is converted to an equivalent load by 
$  applying x-force resultants to the nodes lying along the right boundary 
$ 
*DEFINE_CURVE 
1,0,0.,0.,0.,0.,0 
0.,0. 
.1,10000. 
*LOAD_NODE_POINT 
100,6,1,1.0 
$ 
*CONSTRAINED_INTERPOLATION 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$     icid      dnid      ddof 
         1       100         5 
$     inid      idof    twghtx    twghty    twghtz    rwghtx    rwghty    rwghtz 
        96       1 
        97       1 
        98       1 
        99       1 
       177       1 
       178       1 
       179       1 
       180       1 
$ 
*......... 
$
*CONSTRAINED_INTERPOLATION_SPOTWELD 
(prior notation *CONSTRAINED_SPR3 still works) 
Purpose:    Define  a  spotweld  with  failure.    This  model  includes  a  plasticity-damage 
model that reduces the force and moment resultants to zero as the spotweld fails.  The 
location  of  the  spotweld  is  defined  by  a  single  node  at  the  center  of  two  connected 
sheets.  The domain of influence is specified by a radius, which should be approximate-
ly equal to the spotweld’s radius.  The algorithm does a normal projection from the two 
sheets  to  the  spotweld  node  and  locates  all nodes  within  the  user-defined  diameter  of 
influence.    The  numerical  implementation  of  this  model  is  similar  to  the  SPR2  model 
(*CONSTRAINED_SPR2). 
  Card 1 
1 
2 
3 
4 
Variable 
PID1 
PID2 
NSID 
THICK 
Type 
I 
I 
I 
F 
5 
R 
F 
6 
7 
8 
STIFF 
ALPHA1  MODEL 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
1.0 
  Card 2 
Variable 
1 
RN 
Type 
F 
2 
RS 
F 
3 
4 
5 
6 
7 
8 
BETA 
LCF 
LCUPF 
LCUPR 
DENS 
INTP 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Additional Card for MODEL = 2, 12, or 22. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
UPFN 
UPFS 
ALPHA2 
BETA2 
UPRN 
UPRS 
ALPHA3 
BETA3 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none
Additional Card for MODEL = 2, 12, or 22. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MRN 
MRS 
Type 
F 
F 
Default 
none 
none 
  VARIABLE   
DESCRIPTION
PID1 
PID2 
NSID 
Part ID of first sheet. 
Part ID of second sheet. 
Node set ID of spotweld location nodes. 
THICK 
Total thickness of both sheets. 
R 
Spotweld radius. 
STIFF 
Elastic stiffness.  Function ID if MODEL > 10. 
ALPHA1 
Scaling factor 𝛼1. Function ID if MODEL > 10. 
MODEL 
Material behavior and damage model, see remarks.  
EQ.  1:  SPR3 (default), 
EQ.  2:  SPR4, 
EQ.11:  same  as  1  with  selected  material  parameters  as
functions,  
EQ.12:  same  as  2  with  selected  material  parameters  as
functions,  
EQ.21:  same as 11 with slight modification, see remarks, 
EQ.22:  same as 12 with slight modification, see remarks. 
RN 
RS 
Tensile strength factor. Function ID if MODEL > 10. 
Shear strength factor. Function ID if MODEL > 10. 
BETA 
Exponent for plastic potential 𝛽1. Function ID if MODEL > 10.
VARIABLE   
DESCRIPTION
LCF 
LCUPF 
LCUPR 
DENS 
INTP 
UPFN 
UPFS 
Load  curve  ID  describing  force  versus  plastic  displacement:
𝐹0(𝑢̅𝑝𝑙). 
Load  curve  ID  describing  plastic  initiation  displacement  versus
𝑝𝑙(𝜅). Only for MODEL = 1, 11, or 21. 
mode mixity: 𝑢̅0
Load  curve  ID  describing  plastic  rupture  displacement  versus
𝑝𝑙(𝜅). Only for MODEL = 1, 11, or 21. 
mode mixity: 𝑢̅𝑓
Spotweld density (necessary for time step calculation). 
Flag for interpolation.  
EQ.0: linear (default),  
EQ.1: uniform, 
EQ.2: inverse distance weighting. 
𝑝𝑙,𝑛 . 
Plastic initiation displacement in normal direction 𝑢̅0,ref
𝑝𝑙,𝑠 . 
Plastic initiation displacement in shear direction 𝑢̅0,ref
ALPHA2 
Plastic initiation displacement scaling factor 𝛼2 . 
BETA2 
UPRN 
UPRS 
Exponent for plastic initiation displacement 𝛽2. 
𝑝𝑙,𝑛 . 
Plastic rupture displacement in normal direction 𝑢̅𝑓 ,ref
𝑝𝑙,𝑠 . 
Plastic rupture displacement in shear direction 𝑢̅𝑓 ,ref
ALPHA3 
Plastic rupture displacement scaling factor 𝛼3 . 
BETA3 
Exponent for plastic rupture displacement 𝛽3. 
Proportionality factor for dependency RN. 
Proportionality factor for dependency RS. 
MRN 
MRS 
Remarks: 
When  this  feature  is  used,  it  is  recommended  to  use  the  drilling  rotation  constraint 
method for the connected components in explicit analysis, i.e.  parameter DRCPSID of
*CONTROL_SHELL  should  refer  to  all  shell  parts 
TION_SPOTWELD connections. 
involved 
in  INTERPOLA-
MODEL = 1, 11, or 21 (“SPR3”) 
This  numerical  model  is  similar  to  the  self-piercing  rivet  model  SPR2    but  with  some  differences  to  make  it  more  suitable  for  spotwelds.  
The  first  difference  is  symmetric  behavior  of  the  spotweld  connection,  i.e.    there  is  no 
distinction  between  a  master  sheet  and  a  slave  sheet.    This  is  done  by  averaging  the 
normals of both parts and by always distributing the balance moments equally to both 
sides.  
The second difference is that there are not only two but three quantities to describe the 
kinematics,  namely  the  normal  relative  displacement  𝛿𝑛,  the  tangential  relative 
displacement 𝛿𝑡, and the relative rotation 𝜔𝑏 - all with respect to the plane-of-maximum 
opening.  I.e.  a relative displacement  vector is defined as 
𝐮 = (𝛿𝑛, 𝛿𝑡, 𝜔𝑏) 
The  third  difference  is  the  underlying  material  model.    With  the  described  kinematic 
quantities, an elastic effective force vector is computed first: 
𝐟 ̃ = (𝑓𝑛, 𝑓𝑡, 𝑚𝑏) = STIFF × 𝐮 = STIFF × (𝜹𝒏, 𝜹𝒕, 𝝎𝒃) 
From that, two resultant forces for normal direction and tangential direction (shear) are 
computed via 
Then, a yield function is defined for plastic behavior 
𝐹𝑛 = ⟨𝑓𝑛⟩ + 𝛼1𝑚𝑏,
𝐹𝑠 = 𝑓𝑡 
𝜙(𝐟 ̃, 𝒖̅pl) = 𝑃(𝐟 ̃) − 𝐹0(𝒖̅pl) ≤ 0 
with relative plastic displacement 𝑢̅𝑝𝑙, potential P 
𝑃(𝐟 ̃) = [(
𝐹𝑛
𝑅𝑛
)
+ (
𝐹𝑠
𝑅𝑠
𝟏/𝜷
]
)
(cid:448)(cid:1377)
(cid:448)(cid:1377)(cid:9)(cid:487)(cid:1135)(cid:981)(cid:10)
(cid:487)(cid:1135)(cid:981)
(cid:1377)
(cid:1377) (cid:12) (cid:487)(cid:1135)(cid:981)
(cid:487)(cid:1135)(cid:981)
(cid:1401)
(cid:487)(cid:1135)(cid:981)
Figure 10-12.  Force-displacement curve: plasticity and linear damage 
and isotropic hardening described by load curve LCF : 
𝐹0 = 𝐹0(𝒖̅pl) 
In addition, a linear softening evolution is incorporated, where damage is defined as: 
pl(𝜅)
𝑑 =
𝑢̅pl − 𝑢̅0
pl(𝜅)
𝑢̅𝑓
,
0 < 𝑑 < 1 
with mode mixity 
𝜅 =
arctan (
𝐹𝑛
𝐹𝑠
) ,       0 < 𝜅 < 1 
Finally, the nominal force is computed as: 
𝐟 = (1 − 𝑑)𝐟 ̃ 
MODEL = 2, 12, or 22 (“SPR4”) 
In this approach, the relative displacement  vector is defined as in model 1 
The elastic effective force vector is computed using the elastic stiffness STIFF 
𝐟 ̃ = (𝑓𝑛, 𝑓𝑡) = STIFF × 𝐮 = STIFF × (𝜹𝒏, 𝜹𝒕) 
𝐮 = (𝛿𝑛, 𝛿𝑡) 
A yield function is defined for plastic behavior 
𝜙(𝐟 ̃, 𝒖̅𝒑𝒍) = 𝑃(𝐟 ̃) − 𝐹0(𝒖̅𝒑𝒍) ≤ 0 
with relative plastic displacement 𝑢̅𝑝𝑙, potential P 
𝑃(𝐟 ̃) = [(
𝑓𝑛
𝑅̃ 𝑛
𝜷𝟏
)
+ (
𝑓𝑡
𝑅̃ 𝑠
𝟏/𝜷𝟏
)
]
wherein  𝑅̃ 𝑛  and  𝑅̃ 𝑠  represents  the  load  capacity  in  normal  and  tangential  direction 
respectively.    They  are  calculated  by  the  values  of  RN  and  RS  and  the  influence  of 
relative rotation angle 𝜔𝑏scaled by ALPHA1 
𝑅̃ 𝑠 = 𝑅𝑠 
𝑅̃ 𝑛 = 𝑅𝑛(1 − 𝛼1 𝜔𝑏) 
In addition, a linear softening evolution is incorporated, where damage is defined as: 
𝑑 =
𝑝𝑙
𝑢̅𝑝𝑙 − 𝑢̅0
𝑝𝑙
𝑢̅𝑓
,
0 < 𝑑 < 1 
The calculation of 𝑢̅0
𝑝𝑙 and 𝑢̅𝑓
𝑝𝑙 is done by solving the following equations 
𝛽2
𝑝𝑙,𝑛
𝑢̅0
⎤
⎡
⎥
⎢
𝑝𝑙,𝑛 (1 − 𝛼2𝜔𝑏)⎦
𝑢̅0,ref
⎣
⎧
{
⎨
{
⎩
+
𝑝𝑙,𝑠
⎜⎜⎜⎛ 𝑢̅0
𝑝𝑙,𝑠
𝑢̅0,𝑟𝑒𝑓
⎝
⎟⎟⎟⎞
⎠
𝛽2
𝛽2
⎫
}
⎬
}
⎭
− 1 = 0 
𝑝𝑙 
𝑝𝑙,𝑛 = sin(𝜑) 𝑢̅0
𝑢̅0
𝑝𝑙 
𝑝𝑙,𝑠 = c𝑜𝑠(𝜑)𝑢̅0
𝑢̅0
𝛽3
𝑝𝑙,𝑛
𝑢̅𝑓
⎤
⎡
⎥
⎢
𝑝𝑙,𝑛 (1 − 𝛼3𝜔𝑏)⎦
𝑢̅𝑓 ,𝑟𝑒𝑓
⎣
⎧
{{
⎨
{{
⎩
+
𝑝𝑙,𝑠
⎜⎜⎜⎛ 𝑢̅𝑓
𝑝𝑙,𝑠
𝑢̅𝑓 ,𝑟𝑒𝑓
⎝
𝛽3
⎟⎟⎟⎞
⎠
𝛽3
⎫
}}
⎬
}}
⎭
− 1 = 0 
considering the load angle 𝜑 
𝑝𝑙 
𝑝𝑙,𝑛 = sin(𝜑) 𝑢̅𝑓
𝑢̅𝑓
𝑝𝑙 
𝑝𝑙,𝑠 = c𝑜𝑠(𝜑)𝑢̅𝑓
𝑢̅𝑓
𝜑 = arctan (
𝑓𝑛
𝑓𝑠
) 
To describe a rate dependent behavior a plastic deformation rate 𝑢̅
̇𝑝𝑙 is defined by 
̇𝑝𝑙 =
𝑢̅
Δ𝑢̅𝑝𝑙
Δ𝑡
wherein    Δ𝑢̅𝑝𝑙  is  the  plastic  increment  in  the  current  time  step  and  Δ𝑡  is  the  time  step 
size.  If MRN and MRS are defined, the calculation of 𝑅̃ 𝑛 and 𝑅̃ 𝑠 is changed to 
𝑅̃ 𝑛(𝑢̅
̇𝑝𝑙) = (𝑅𝑛 + 𝑚𝑅𝑛𝑢̅
̇𝑝𝑙)(1 − 𝛼1 𝜔𝑏)
̇𝑝𝑙) = 𝑅𝑠 + 𝑚𝑅𝑠𝑢̅
A detailed description of the SPR4 approach (MODEL = 2) is given in Bier and Sommer 
[2013], where this model is called “SPR3_IWM”. 
𝑅̃ 𝑠(𝑢̅
̇𝑝𝑙 
MODEL > 10 
If  MODEL  is  chosen  to  be  greater  than  10,  then  5  variables  have  to  be  defined  as 
function  IDs:  STIFF,  ALPHA1,  RN,  RS,  and  BETA.    These  functions  incorporate  the 
following  input  values:  thicknesses  of  both  weld  partners  (t1,  t2)  and  maximum 
engineering  yield  stresses,  also  called  necking  points  (sm1,  sm2).    For  ALPHA1 = 100 
such a function could look like, 
*DEFINE_FUNCTION 
        100 
 func(t1,t2,sm1,sm2)=sm1/sm2 
(This  function  is  only  a  demonstration,  it  does  not  make  any  physical  sense).    For 
MODEL = 11 or 12, the master part is the first weld partner represented by t1 and sm1.  
For  MODEL = 21  or  22,  the  thinner  part  is  the  first  weld  partner.    Since  material 
parameters  have  to  be  identified  from  both  weld  partners  during  initialization,  this 
feature is only available for a subset of material models at the moment, namely no.  24, 
120, 123, and 124.
*CONSTRAINED_JOINT_OPTION_{OPTION}_{OPTION}_{OPTION} 
Available forms include (one is mandatory): 
*CONSTRAINED_JOINT_SPHERICAL 
*CONSTRAINED_JOINT_REVOLUTE 
*CONSTRAINED_JOINT_CYLINDRICAL 
*CONSTRAINED_JOINT_PLANAR 
*CONSTRAINED_JOINT_UNIVERSAL 
*CONSTRAINED_JOINT_TRANSLATIONAL 
*CONSTRAINED_JOINT_LOCKING 
*CONSTRAINED_JOINT_TRANSLATIONAL_MOTOR 
*CONSTRAINED_JOINT_ROTATIONAL_MOTOR 
*CONSTRAINED_JOINT_GEARS 
*CONSTRAINED_JOINT_RACK_AND_PINION 
*CONSTRAINED_JOINT_CONSTANT_VELOCITY 
*CONSTRAINED_JOINT_PULLEY 
*CONSTRAINED_JOINT_SCREW 
If the force output data is to be transformed into a local coordinate use the option: 
LOCAL 
to define a joint ID and heading the following option is available: 
ID 
and to define failure for penalty-based joints (LMF = 0 in *CONTROL_RIGID) use: 
FAILURE 
The ordering of the bracketed options is arbitrary. 
Purpose:  Define a joint between two rigid bodies.
*CONSTRAINED 
Card 1: 
required for all joint types 
Card 2: 
required for joint types: MOTOR, GEARS, RACK_AND_PINION, 
PULLEY, and SCREW 
  Optional Card: 
required only if LOCAL is specified in the keyword 
In the first seven joint types above excepting the Universal joint, the nodal points within 
the nodal pairs (1, 2), (3, 4), and (5, 6)  should coincide 
in  the  initial  configuration,  and  the  nodal  pairs  should  be  as  far  apart  as  possible  to 
obtain the best behavior.  For the Universal Joint the nodes within the nodal pair (3, 4) 
do  not  coincide,  but  the  lines  drawn  between  nodes  (1, 3)  and  (2, 4)  must  be 
perpendicular. 
For the Gear joint the nodes within the nodal pair (1, 2) must not coincide. 
When  the  penalty  method  is  used  ,  at  each  time  step,  the 
relative penalty stiffness is multiplied by a function dependent on the step size to give 
the  maximum  stiffness  that  will  not  destroy  the  stability  of  the  solution.    Instabilities 
can result in the explicit time integration scheme if the penalty stiffness is too large.  If 
instabilities occur, the recommended way to eliminate these problems is to decrease the 
time step or reduce the scale factor on the penalties. 
For cylindrical joints, by setting node 3 to zero, it is possible to use a cylindrical joint to 
join a node that is not on a rigid body (node 1) to a rigid body (nodes 2 and 4). 
ID Card.  Additional card for ID keyword option.  
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
JID 
Type 
I 
HEADING 
A70 
The  heading  is  picked  up  by  some  of  the  peripheral  LS-DYNA  codes  to  aid  in  post-
processing. 
  VARIABLE   
DESCRIPTION
JID 
Joint ID.  This must be a unique number. 
HEADING 
Joint descriptor.  It is suggested that unique descriptions be used.
Card 1 
Variable 
Type 
Default 
1 
N1 
I 
0 
2 
N2 
I 
0 
3 
N3 
I 
0 
4 
N4 
I 
0 
5 
N5 
I 
0 
6 
N6 
I 
0 
7 
8 
RPS 
DAMP 
F 
F 
1.0 
1.0 
  VARIABLE   
DESCRIPTION
N1 
N2 
N3 
N4 
N5 
N6 
Node 1, in rigid body A.  Define for all joint types. 
Node 2, in rigid body B.  Define for all joint types. 
Node  3,  in  rigid  body  A.    Define  for  all  joint  types  except
SPHERICAL. 
Node  4,  in  rigid  body  B.    Define  for  all  joint  types  except
SPHERICAL. 
Node 5, in rigid body A.  Define for joint types TRANSLATION-
AL, LOCKING, ROTATIONAL_MOTOR, CONSTANT_VELOCI-
TY, GEARS, RACK_AND_PINION, PULLEY, and SCREW 
Node 6, in rigid body B.  Define for joint types TRANSLATION-
AL, LOCKING, ROTATIONAL_MOTOR, CONSTANT_VELOCI-
TY, GEARS, RACK_AND_PINION, PULLEY, and SCREW 
RPS 
Relative penalty stiffness (default = 1.0):  
GT.0.0: constant value, 
LT.0.0:  time dependent value given by load curve ID = -RPS 
(only  for  SPHERICAL,  REVOLUTE,  and  CYLINDRI-
CAL). 
DAMP 
Damping  scale  factor  on  default  damping  value.    (Revolute  and
Spherical Joints): 
EQ.0.0: 
default is set to 1.0, 
GT.0.0.AND.LE.0.01: no damping is used.
Rotational  Properties  Card.    Additional  card  for  joint  types  MOTOR,  GEARS, 
RACK_AND_PINION, PULLEY, and SCREW.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PARM 
LCID 
TYPE 
R1 
H_ANGLE
Type 
F 
I 
I 
F 
F 
Default 
none 
0.0 
  VARIABLE   
DESCRIPTION
PARM 
Parameter, which a function of joint type: 
Gears:  define 𝑅2/𝑅1 
  Rack and Pinion:  define ℎ 
Pulley:  define 𝑅2/𝑅1 
Screw:  define 𝑥̇/𝜔 
Motors:  leave blank 
Define load curve ID for MOTOR joints. 
Define integer flag for MOTOR joints as follows: 
EQ.0: translational/rotational velocity 
EQ.1: translational/rotational acceleration 
EQ.2: translational/rotational displacement 
Radius,  𝑅1,  for  the  gear  and  pulley  joint  type.    If  left  undefined,
nodal points 5 and 6 are assumed to be on the outer radius.  The 
value  of  R1  and  R2  affect  the  reaction  forces  written  to  output.
The forces are calculated from the moments by dividing them by
the radii. 
LCID 
TYPE 
R1 
H_ANGLE 
Helix angle in degrees.  This is only necessary for the gear joint if
the gears do not mesh tangentially, e.g., worm gears, see remarks
below for a definition.
Local Card.  Additional card required for LOCAL keyword option.  
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RAID 
LST 
Type 
Default 
I 
0 
I 
0 
  VARIABLE   
RAID 
DESCRIPTION
Rigid  body  or  accelerometer  ID.    The  force  resultants  are  output
in the local system of the rigid body or accelerometer. 
LST 
Flag for local system type: 
EQ.0: rigid body 
EQ.1: accelerometer 
Failure Card 1.  Additional card for FAILURE keyword option.  
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CID 
TFAIL 
COUPL 
Type 
Default 
I 
0 
F 
0 
F 
0. 
Failure Card 2.  Additional card for FAILURE keyword option.  
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NXX 
NYY 
NZZ 
MXX 
MYY 
MZZ 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F
VARIABLE   
CID 
DESCRIPTION
Coordinate  ID  for  resultants  in  the  failure  criteria.    If  zero,  the
global coordinate system is used. 
TFAIL 
Time for joint failure.  If zero, joint never fails. 
COUPL 
NXX 
NYY 
NZZ 
MXX 
MYY 
MZZ 
Coupling  between  the  force  and  moment  failure  criteria.    If
COUPL is less than or equal to zero, the failure criteria is identical
to  the  spotwelds.    When  COUPL  is  greater  than  zero,  the  force
and  moment  results  are  considered  independently.    See  the
remark below. 
Axial  force  resultant  𝑁𝑥𝑥𝐹at  failure.    If  zero,  failure  due  to  this 
component is not considered. 
Force  resultant  𝑁𝑦𝑦𝐹  at  failure.    If  zero,  failure  due  to  this 
component is not considered. 
Force  resultant  𝑁𝑧𝑧𝐹  at  failure.    If  zero,  failure  due  to  this 
component is not considered. 
Torsional moment resultant 𝑀𝑧𝑧𝐹 at failure.  If zero, failure due to 
this component is not considered. 
Moment  resultant  𝑀𝑦𝑦𝐹  at  failure.    If  zero,  failure  due  to  this
component is not considered. 
Moment  resultant  𝑀𝑧𝑧𝐹  at  failure.    If  zero,  failure  due  to  this 
component is not considered.
Node 2 at
center
The axial
direction, e1
The tangential
direction, e2
Tangent vector 
to the teeth e3
Figure 10-13.  Helix angle 𝛼 definition, gear #2 viewed from the extension of
node 𝑛2 to node 𝑛6. 
Remarks: 
The  moments  for  the  revolute,  cylindrical,  planar,  translational,  and  locking  joints  are 
calculated  at  the  midpoint  of  nodes  N1  and  N3.    The  moments  for  the  spherical, 
universal,  constant  velocity,  gear,  pulley,  and  rack  and  pinion  joints  are  calculated  at 
node N1.  When COUPL is less than or equal to zero, the failure criteria is 
(
𝑁𝑥𝑥
𝑁𝑥𝑥𝐹
)
+ (
𝑁𝑦𝑦
𝑁𝑦𝑦𝐹
)
+ (
𝑁𝑧𝑧
𝑁𝑧𝑧𝐹
)
+ (
𝑀𝑥𝑥
𝑀𝑥𝑥𝐹
)
+ (
𝑀𝑦𝑦
𝑀𝑦𝑦𝐹
)
+ (
𝑀𝑧𝑧
𝑀𝑧𝑧𝐹
)
− 1 = 0. 
Otherwise, it consists of both 
and 
(
𝑁𝑥𝑥
𝑁𝑥𝑥𝐹
)
+ (
𝑁𝑦𝑦
𝑁𝑦𝑦𝐹
)
+ (
𝑁𝑧𝑧
𝑁𝑧𝑧𝐹
)
− 1 = 0, 
(
𝑀𝑥𝑥
𝑀𝑥𝑥𝐹
)
+ (
𝑀𝑦𝑦
𝑀𝑦𝑦𝐹
)
+ (
𝑀𝑧𝑧
𝑀𝑧𝑧𝐹
)
− 1 = 0. 
For a gear joint, the relative direction and magnitude of rotation between the two gears 
is determined by the helix angle.  Let  𝐞1 be the unit normal directed from node 2 to 4, 
which  corresponds  to  the  second  gear’s  rotation  axis.    See  Figure  10-23.    Let   𝐞2  be 
defined  as  the  positively  oriented  tangent  vector  to  motion  of  the  teeth  when  spun 
about the 𝐞1 axis (the gear’s axis).  See Figure 10-13.  The helix angle 𝛼 characterizes the
deviation  of  the  teeth  axis  from  the  gear  axis.    In  particular,  𝛼  is  defined  as  the  angle 
between the direction of teeth, called 𝐞3, and the axis of the gear  𝐞1, 
𝐞3 = cos𝛼𝐞1 + sin𝛼𝐞2. 
The  gears  are  assumed  to  be  setup  so  that  the  teeth  initially  fit  having  matching  𝐞3 
directions.  A nonzero helix angle is typically used to model worm gears.
1,2
Radial cross section
Figure  10-14.    Spherical  joint.    The  relative  motion  of  the  rigid  bodies  is
constrained so that nodes which are initially coincident remain coincident.  In
the above figure the socket’s node is not interior to the socket—LS-DYNA does 
not require that a rigid body’s nodes be interior to the body. 
Centerline
Centerline
3,4
1,2
Figure  10-15.   Revolute Joint.  Nodes  1 and 2 are  coincident; nodes  3 and 4 are
coincident.  Nodes 1 and 3 belong to rigid body A; nodes 2 and 4 belong to rigid
body  B.    The  relative  motion  of  the  two  rigid  bodies  is  restricted  to  rotations
about the axis formed by the two pairs of coincident nodes.  This axis is labeled 
the “centerline”.
Initial
Current
Centerline
1,2
3,4
Figure 10-16.  Cylindrical Joint.  This joint is derived from the rotational joint by
relaxing the constraints along the centerline.  This joint admits relative rotation 
and translation along the centerline. 
Initial
Current
Centerline
1,2
3,4
5,6
Figure 10-17.  Translational joint.  This is a cylindrical joint with a third pair of
off-centerline  nodes  which  restrict  rotation.    Aside  from  translation  along  the
centerline, the two rigid bodies are stuck together.
Figure  10-18.    Planar  joint.    This  joint  is  derived  from  the  rotational  joint  by
relaxing the constraints normal to the centerline.  Relative displacements along
the direction of the centerline are excluded. 
1,2
Figure  10-19.    Universal  Joint.    Nodes  1  and  2  are  initially  coincident.    The
segments formed by nodal pairs (1, 3) and (2, 4) must be orthogonal; they serve
as  axes  about  which  the  two  bodies  may  undergo  relative  rotation.    The
universal  joint  excludes  all  other  relative  motion  and  the  axes  remain
orthogonal at all time.
Initial, Final
1,2
5,6
3,43,4
Figure 10-20.  Locking Joint.  A locking joint couples two rigid bodies in all six
degrees-of-freedom.    The  forces  and  moments  required  to  form  this  coupling
are  written  to  the  jntforc  file  (*DATABASE_JNTFORC).    As  stated  in  the
Remarks,  forces  and  moments  in  jntforc  are  calculated  halfway  between  N1
and  N3.    Nodal  pairs  (1, 2),  (3, 4)  and  (5, 6)  must  be  coincident.    The  three
spatial  points  corresponding  to  three  nodal  pairs  must  be  neither  collocated
nor collinear. 
Centerline
†
Load Curve
Time
Figure  10-21.    Translational  motor  joint.    This  joint  is  usually  used  in
combination  with  a  translational  or  a  cylindrical  joint.    Node  1  and  node  2
belong  to  the  first  rigid  body  and  the  second  rigid  body,  resp.    Furthermore,
nodes  1  and  2  must  be  coincident.    Node  3  may  belong  to  either  rigid  body. 
The vector from node 2 to node 3 is the direction of relative motion.  Node 4 is
not used and can be left blank.  The value of the load curve may specify any of
several kinematic measures; see TYPE.
Load curve defines relative
rotational motion in radians
per unit time.
Figure  10-22.    Rotational  motor  joint.    This  joint  can  be  used  in  combination
with other joints such as the revolute or cylindrical joints. 
Node 1 at
center
R1
R2
Node 1 at
center
Node 2 at
center
R2
Node 2 at
center
R1
Figure  10-23.    Gear  joints.    Nodal  pairs  (1, 3)  and  (2, 4)  define  axes  that  are
orthogonal to the gears.  Nodal pairs (1, 5) and (2, 6) define vectors in the plane
of the gears.  The ratio 𝑅2 𝑅1⁄
 is specified but need not necessarily correspond
to  the geometry,  if  for  instance  the  gear  consists  of  spiral  grooves.    Note  that
the  gear  joint  in  itself  does  not  maintain  the  contact  point  but  this  requires
additional treatment, such as accompanying it with other joints.
Node 1 at the
center of the pinion
Node 2 inside
the rack
Figure 10-24.  Rack and pinion joint.  Nodal pair (1, 3) defines the axis of 
rotation  of  the  first  body  (the  pinion).    Nodal  pair  (1, 5)  is  a  vector  in  the 
plane of the pinion and is orthogonal to nodal pair (1, 3).  Nodal pair (2, 4) 
defines  the  direction  of  travel  for the  second  body  (the  rack).    Nodal  pair 
(2, 6)  is  parallel to the axis  of the  pinion and  is thus parallel  to nodal pair
(1, 3).  The value h is specified.  The velocity of the rack is ℎ𝜔pinion. 
1 2
Figure  10-25.   Constant velocity  joint.    Nodal pairs  (1, 3) and (2, 4) define an
axes  for  the  constant  angular  velocity,  and  nodal  pairs  (1, 5)  are  orthogonal
vectors.  Here nodal points 1 and 2 must be coincident.
R2
R1
Node 1
at Center
Node 2 at Center
Figure  10-26.    Pulley  joint.    Nodal  pairs  (1, 3)  and  (2, 4)  define  axes  that  are 
orthogonal  to  the  pulleys.    Nodal  pairs  (1, 5)  and  (2, 6)  define  vectors  in  the 
plane of the pulleys.  The ratio 𝑅2 𝑅1⁄
 is specified.
Screw Centerline
1,2 
5,6
3,4
Figure 10-27.  Screw joint.  The second body translates in response to the spin
of the first body.  Nodal pairs (1, 3) and (2, 4) lie along the same axis and nodal 
pairs (1, 5) and (2, 6) are orthogonal vectors.  The helix ratio, 𝑥̇
𝜔⁄ , is specified.
*CONSTRAINED_JOINT 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *CONSTRAINED_JOINT_PLANAR 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Define a planar joint between two rigid bodies. 
$    - Nodes 91 and 94 are on rigid body 1. 
$    - Nodes 21 and 150 are on rigid body 2. 
$    - Nodes 91 and 21 must be coincident. 
$        * These nodes define the origin of the joint plane. 
$    - Nodes 94 and 150 must be coincident. 
$        * To accomplish this, massless node 150 is artificially created at 
$           the same coordinates as node 94 and then added to rigid body 2. 
$        * These nodes define the normal of the joint plane (e.g., the 
$           vector from node 91 to 94 defines the planes' normal). 
$ 
*CONSTRAINED_JOINT_PLANAR 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$       n1        n2        n3        n4        n5        n6       rps 
        91        21        94       150                     0.000E+00 
$ 
$ 
*NODE 
$    nid               x               y               z      tc      rc 
     150            0.00            3.00            0.00       0       0 
$ 
*CONSTRAINED_EXTRA_NODES_SET 
$      pid      nsid 
         2         6 
$*SET_NODE_LIST 
$      sid 
         6 
$     nid1 
       150 
$ 
$$$  request output for joint force data 
$ 
*DATABASE_JNTFORC 
$  dt/cycl      lcdt 
    0.0001 
$ 
Example 2: 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *CONSTRAINED_JOINT_REVOLUTE 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Create a revolute joint between two rigid bodies.  The rigid bodies must 
$  share a common edge to define the joint along.  This edge, however, must 
$  not have the nodes merged together.  Rigid bodies A and B will rotate  
$  relative to each other along the axis defined by the common edge. 
$ 
$  Nodes 1 and 2 are on rigid body A and coincide with nodes 9 and 10 
$  on rigid body B, respectively.  (This defines the axis of rotation.) 
$
$  The relative penalty stiffness on the revolute joint is to be 1.0, 
$ 
*CONSTRAINED_JOINT_REVOLUTE 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$       n1        n2        n3        n4        n5        n6       rps      damp 
         1         9         2        10                           1.0 
$ 
$  Note:  A joint stiffness is not mandatory for this joint to work.   
$         However, to see how a joint stiffness can be defined for this  
$         particular joint, see the corresponding example listed in:  
$            *CONSTRAINED_JOINT_STIFFNESS_GENERALIZED 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$
*CONSTRAINED_JOINT_COOR_OPTION_{OPTION}_{OPTION}_{OPTION} 
Available forms include (one is mandatory): 
*CONSTRAINED_JOINT_COOR_SPHERICAL 
*CONSTRAINED_JOINT_COOR_REVOLUTE 
*CONSTRAINED_JOINT_COOR_CYLINDRICAL 
*CONSTRAINED_JOINT_COOR_PLANAR 
*CONSTRAINED_JOINT_COOR_UNIVERSAL 
*CONSTRAINED_JOINT_COOR_TRANSLATIONAL 
*CONSTRAINED_JOINT_COOR_LOCKING 
*CONSTRAINED_JOINT_COOR_TRANSLATIONAL_MOTOR 
*CONSTRAINED_JOINT_COOR_ROTATIONAL_MOTOR 
*CONSTRAINED_JOINT_COOR_GEARS 
*CONSTRAINED_JOINT_COOR_RACK_AND_PINION 
*CONSTRAINED_JOINT_COOR_CONSTANT_VELOCITY 
*CONSTRAINED_JOINT_COOR_PULLEY 
*CONSTRAINED_JOINT_COOR_SCREW 
If the force output data is to be transformed into a local coordinate use the option: 
LOCAL 
to define a joint ID and heading the following option is available: 
ID 
and to define failure for penalty-based joints (LMF = 0 in *CONTROL_RIGID) use: 
FAILURE 
The ordering of the bracketed options is arbitrary.  
Purpose:    Define  a  joint  between  two  rigid  bodies,  see  Figure.    The  connection 
coordinates  are  given  instead  of  the  nodal  point  IDs  required  in  the  previous  section, 
*CONSTRAINED_JOINT_{OPTION}.      Nodes  are  automatically  generated  for  each
coordinate and are constrained to the rigid body.  Where coincident nodes are expected 
in  the  initial  configuration,  only  one  connection  coordinate  is  needed  since  the 
connection coordinate for the second node, if given, is ignored.  The created nodal ID’s 
are  chosen  to  exceed  the  maximum  user  ID.    The  coordinates  of  the  joint  nodes  are 
specified  on  Cards  2 - 7.    The  input  which  follows  Card  7  is  identical  to  that  in  the 
previous section. 
Card Format: 
Cards 1 - 7: 
required for all joint types 
Card 8: 
required for joint types: MOTOR, GEARS, RACK_AND_PINION, 
PULLEY, and SCREW 
  Optional Card: 
required when LOCAL is specified in the keyword 
In the first seven joint types above excepting the Universal joint, the coordinate points 
within  the  nodal  pairs  (1, 2),  (3, 4),  and  (5, 6)    should 
coincide  in  the  initial  configuration,  and  the  nodal  pairs  should  be  as  far  apart  as 
possible  to  obtain  the  best  behavior.    For  the  Universal  Joint  the  nodes  within  the 
coordinate pair (3, 4) do not coincide, but the lines drawn between nodes (1, 3) and (2, 4) 
must be perpendicular. 
For the Gear joint the nodes within the coordinate pair (1, 2) must not coincide. 
When  the  penalty  method  is  used  ,  at  each  time  step,  the 
relative penalty stiffness is multiplied by a function dependent on the step size to give 
the  maximum  stiffness  that  will  not  destroy  the  stability  of  the  solution.    LS-DYNA’s 
explicit time integrator can become unstable when the penalty stiffness is too large.  If 
instabilities occur, the recommended way to eliminate these problems is to decrease the 
time step or reduce the scale factor on the penalties. 
For cylindrical joints, by setting node 3 to zero, it is possible to use a cylindrical joint to 
join a node that is not on a rigid body (node 1) to a rigid body (nodes 2 and 4). 
ID Card.  Additional card for the ID keyword option.  
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
JID 
Type 
I 
HEADING 
A70 
The  heading  is  picked  up  by  some  of  the  peripheral  LS-DYNA  codes  to  aid  in  post-
processing.
VARIABLE   
DESCRIPTION
JID 
Joint ID.  This must be a unique number. 
HEADING 
Joint descriptor.  It is suggested that unique descriptions be used.
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RBID_A 
RBID_B 
RPS 
DAMP 
TMASS 
RMASS 
Type 
I 
I 
F 
  Card 2 
Variable 
1 
X1 
Type 
F 
  Card 3 
Variable 
1 
X2 
Type 
F 
  Card 4 
Variable 
1 
X3 
Type 
F 
2 
Y1 
F 
2 
Y2 
F 
2 
Y3 
F 
3 
Z1 
F 
3 
Z2 
F 
3 
Z3 
F 
F 
4 
F 
5 
F 
6 
7 
8 
4 
5 
6 
7 
8 
4 
5 
6 
7
Card 5 
Variable 
1 
X4 
Type 
F 
  Card 6 
Variable 
1 
X5 
Type 
F 
  Card 7 
Variable 
1 
X6 
Type 
F 
2 
Y4 
F 
2 
Y5 
F 
2 
Y6 
F 
3 
Z4 
F 
3 
Z5 
F 
3 
Z6 
F 
4 
5 
6 
7 
8 
4 
5 
6 
7 
8 
4 
5 
6 
7 
8 
  VARIABLE   
DESCRIPTION
RBID_A 
Part ID of rigid body A. 
RBID_B 
Part ID of rigid body B. 
RPS 
Relative penalty stiffness (default = 1.0). 
DAMP 
Damping  scale  factor  on  default  damping  value.    (Revolute  and
Spherical Joints): 
EQ.0.0: 
default is set to 1.0, 
GT.0.0 and LE.0.01:  no damping is used. 
TMASS 
RMASS 
Lumped  translational  mass.    The  mass  is  equally  split  between
the first points defined for rigid bodies A and B. 
Lumped  rotational  inertia.    The  inertia  is  equally  split  between
the first points defined for rigid bodies A and B. 
X1, Y1, Z1 
Coordinate of point 1, in rigid body A.  Define for all joint types.
VARIABLE   
X2, Y2, Z2 
DESCRIPTION
Coordinate  of    point  2,  in  rigid  body  B.    If  points  1  and  2  are
coincident in the specified joint type, the coordinate for point 1 is
used. 
X3, Y3, Z31 
Coordinate of point 3, in rigid body A.  Define for all joint types. 
X4, Y4, Z4 
Coordinate  of    point  4,  in  rigid  body  B.    If  points  3  and  4  are
coincident in the specified joint type, the coordinate for point 3 is
used. 
X5, Y5, Z5 
Coordinate of point 5, in rigid body A.  Define for all joint types. 
X6, Y6, Z6 
Coordinate  of    point  6,  in  rigid  body  B.    If  points  5  and  6  are
coincident in the specified joint type, the coordinate for point 5 is
used. 
Rotational  Properties  Card.    Additional  card  for  joint  types  MOTOR,  GEARS, 
RACK_AND_PINION, PULLEY, and SCREW. 
5 
6 
7 
8 
  Card 8 
1 
2 
3 
Variable 
PARM 
LCID 
TYPE 
Type 
F 
I 
I 
4 
R1 
F 
Default 
none 
  VARIABLE   
DESCRIPTION
PARM 
Parameter, which a function of joint type: 
Gears:  define 𝑅2/𝑅1 
  Rack and Pinion:  define ℎ 
Pulley:  define 𝑅2/𝑅1 
Screw:  define 𝑥̇/𝜔 
Motors:  leave blank 
LCID 
Define load curve ID for MOTOR joints.
VARIABLE   
DESCRIPTION
TYPE 
Define integer flag for MOTOR joints as follows: 
EQ.0: translational/rotational velocity 
EQ.1: translational/rotational acceleration 
EQ.2: translational/rotational displacement 
R1 
Radius,  𝑅1,  for  the  gear  and  pulley  joint  type.    If  left  undefined,
nodal points 5 and 6 are assumed to be on the outer radius.  R1 is
the  moment  arm  that  goes  into  calculating  the  joint  reaction 
forces.    The  ratio  R2/R1  gives  the  transmitted  moments,  but  not
the forces.  The force is moment divided by distance R1. 
Local Card.  Additional card for LOCAL keyword option.  
  Card 9 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RAID 
LST 
Type 
Default 
I 
0 
I 
0 
  VARIABLE   
RAID 
DESCRIPTION
Rigid  body  or  accelerometer  ID.    The  force  resultants  are  output
in the local system of the rigid body or accelerometer. 
LST 
Flag for local system type: 
EQ.0: rigid body 
EQ.1: accelerometer
Failure Card 1.  Additional card for the FAILURE keyword option.  
  Card 10 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CID 
TFAIL 
COUPL 
Type 
Default 
I 
0 
F 
0 
F 
0. 
Failure Card 2.  Additional card for the FAILURE keyword option. 
  Card 11 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NXX 
NYY 
NZZ 
MXX 
MYY 
MZZ 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
  VARIABLE   
CID 
DESCRIPTION
Coordinate  ID  for  resultants  in  the  failure  criteria.    If  zero,  the
global coordinate system is used. 
TFAIL 
Time for joint failure.  If zero, joint never fails. 
COUPL 
NXX 
NYY 
NZZ 
Coupling between the force and moment failure criteria.  If COU-
PL  is  less  than  or  equal  to  zero,  the  failure criteria  is  identical to
the spotwelds.  When COUPL is greater than zero, the force and 
moment results are considered independently.  See the remarks in
*CONSTRAINED_JOINT_{OPTION}. 
Axial  force  resultant  𝑁𝑥𝑥𝐹at  failure.    If  zero,  failure  due  to  this 
component is not considered. 
Force  resultant  𝑁𝑌𝑌𝐹  at  failure.    If  zero,  failure  due  to  this 
component is not considered. 
Force  resultant  𝑁𝑧𝑧𝐹  at  failure.    If  zero,  failure  due  to  this 
component is not considered.
VARIABLE   
DESCRIPTION
MXX 
MYY 
MZZ 
Torsional  moment  resultant  𝑀𝑋𝑋𝐹  at  failure.    If  zero,  failure  due 
to this component is not considered. 
Moment  resultant  𝑀𝑌𝑌𝐹  at  failure.    If  zero,  failure  due  to  this 
component is not considered. 
Moment  resultant  𝑀𝑍𝑍𝐹  at  failure.    If  zero,  failure  due  to  this 
component is not considered.
*CONSTRAINED_JOINT_STIFFNESS_OPTION_{OPTION} 
Available options include: 
FLEXION-TORSION 
GENERALIZED 
TRANSLATIONAL 
If desired a description of the joint stiffness can be provided with the option: 
TITLE 
which is written into the d3hsp and jntforc files. 
Purpose:  Define optional rotational and translational joint stiffness for joints defined by 
*CONSTRAINED_JOINT_OPTION.    These  definitions  apply  to  all  joints  even  though 
degrees  of  freedom  that  are  considered  in  the  joint  stiffness  capability  may  be 
constrained out in some joint types.  The energy that is dissipated with the joint stiffness 
option is written for each joint in  joint force file with the default  name, jntforc.  In the 
global energy balance this energy is included with the energy of the discrete elements, 
i.e., the springs and dampers. 
Card Format: 
The optional TITLE card and card 1 are common to all joint stiffness types. 
Cards 2 to 4 are unique for each stiffness type. 
Title Card.  Additional card for the TITLE keyword option.  
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
TITLE 
A80
Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
JSID 
PIDA 
PIDB 
CIDA 
CIDB 
JID 
Type 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
CIDA 
none 
  VARIABLE   
DESCRIPTION
TITLE 
Description of joint stiffness for output files jntforc and d3hsp. 
JSID 
PIDA 
PIDB 
CIDA 
CIDB 
Joint stiffness ID 
Part ID for rigid body A, see *PART. 
Part ID for rigid body B, see *PART. 
Coordinate  ID  for  rigid  body  A,  see  *DEFINE_COORDINATE_-
OPTION.    For  the  translational  stiffness  the  local  coordinate
system  must  be  defined  by  nodal  points,  *DEFINE_COORDI-
NATE_NODES,  since  the  first  nodal  point  in  each  coordinate
system is used to track the motion. 
Coordinate  ID  for  rigid  body  B.    If  zero,  the  coordinate  ID  for
rigid  body  A  is  used,  see  *DEFINE_COORDINATE_OPTION. 
For the translational stiffness the local coordinate system must be
defined  by  nodal  points,  *DEFINE_COORDINATE_NODES, 
since  the  first  nodal  point  in  each  coordinate  system  is  used  to
track the motion. 
JID 
Joint ID for the joint reaction forces.  If zero, tables can’t be used
in place of load curves for defining the frictional moments.
Card 2 for FLEXION-TORSION option. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCIDAL 
LCIDG 
LCIDBT  DLCIDAL  DLCIDG  DLCIDBT 
Type 
I 
I 
I 
I 
I 
I 
Default 
none 
1.0 
none 
none 
1.0 
none 
Card 3 for FLEXION-TORSION option. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ESAL 
FMAL 
ESBT 
FMBT 
Type 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
Card 4 for FLEXION-TORSION option. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SAAL 
NSABT 
PSABT 
Type 
F 
F 
F 
Default  not used  not used  not used
Figure 10-28.  The angles 𝛼, 𝛽, 𝛾 align rigid body one with rigid body two for
the FLEXION-TORSION option. 
  VARIABLE   
LCIDAL 
LCIDG 
LCIDBT 
DLCIDAL 
DLCIDG 
DESCRIPTION
Load  curve  ID  for  𝛼-moment  versus  rotation  in  radians.    See 
Figure 10-28 where it should be noted that 0 ≤ 𝛼 ≤ 𝜋.  If zero, the 
applied moment is set to zero.  See *DEFINE_CURVE. 
Load curve ID for 𝛾 versus a scale factor which scales the bending 
moment due to the 𝛼 rotation.  This load curve should be defined 
in the interval −𝜋 ≤ 𝛾 ≤ 𝜋.  If zero the scale factor defaults to 1.0. 
See *DEFINE_CURVE. 
Load  curve  ID  for  𝛽-torsion  moment  versus  twist  in  radians.    If 
zero the applied twist is set to zero.  See *DEFINE_CURVE. 
Load  curve  ID  for  𝛼-damping  moment  versus  rate  of  rotation  in 
radians  per  unit  time.    If  zero,  damping  is  not  considered.    See
*DEFINE_CURVE. 
Load  curve  ID  for 𝛾-damping  scale  factor  versus  rate  of  rotation 
in  radians  per  unit  time.    This  scale  factor  scales  the  𝛼-damping 
moment.  If zero, the scale factor defaults to one.  See *DEFINE_-
CURVE. 
DLCIDBT 
Load curve ID for 𝛽-damping torque versus rate of twist.  If zero 
damping is not considered.  See *DEFINE_CURVE.
z1
z2
y2
x1
y1
x2
Figure 10-29.  Flexion-torsion joint angles.  If the initial positions of the local
coordinate axes of the two rigid bodies connected by the joint do not coincide,
the  angles,  𝛼  and    𝛾,  are  initialized  and  torques  will  develop  instantaneously
based on the defined load curves.  The angle 𝛽 is also initialized but no torque
will  develop  about  the  local  axis  on  which  𝛽  is  measured.    Rather,  𝛽  will  be
measured relative to the computed offset. 
  VARIABLE   
ESAL 
FMAL 
DESCRIPTION
Elastic  stiffness  per  unit  radian  for  friction  and  stop  angles  for  𝛼
rotation.    If  zero,  friction  and  stop  angles  are  inactive  for  𝛼
rotation.  See Figure 10-31. 
Frictional moment limiting value for 𝛼 rotation.  If zero, friction is 
inactive for 𝛼 rotation.  This option may also be thought of as an
elastic-plastic  spring.    If  a  negative  value  is  input  then  the 
absolute value is taken as the load curve or table ID defining the
yield  moment  versus  𝛼  rotation.    A  table  permits  the  moment  to 
also  be  a  function  of  the  joint  reaction  force  and  requires  the
specification of JID on Card 1.  See Figure 10-31.
VARIABLE   
DESCRIPTION
ESBT 
FMBT 
Elastic  stiffness  per  unit  radian  for  friction  and  stop  angles  for 𝛽
twist.  If zero, friction and stop angles are inactive for 𝛽 twist. 
Frictional  moment  limiting  value  for  𝛽  twist.    If  zero,  friction  is 
inactive  for  𝛽  twist.    This  option  may  also  be  thought  of  as  an
elastic-plastic  spring.    If  a  negative  value  is  input  then  the
absolute value is taken as the load curve or table ID defining the
yield  moment versus  𝛽 rotation.   A table  permits  the  moment to 
also  be  a  function  of  the  joint  reaction  force  and  requires  the
specification of JID on Card 1. 
SAAL 
Stop angle in degrees for 𝛼 rotation where 0 ≤ 𝛼 ≤ 𝜋.  Ignored if 
zero.  See Figure 10-31. 
NSABT 
Stop angle in degrees for negative 𝛽 rotation.  Ignored if zero. 
PSABT 
Stop angle in degrees for positive 𝛽 rotation.  Ignored if zero. 
Remarks: 
This option simulates a flexion-torsion behavior of a joint in a slightly different fashion 
than with the generalized joint option. 
After the stop angles are reached the torques increase linearly to resist further angular 
motion using the stiffness values on Card 3.  If the stiffness value is too low or zero, the 
stop will be violated. 
The  moment  resultants  generated  from  the  moment  versus  rotation  curve,  damping 
moment versus rate-of-rotation curve, and friction are evaluated independently and are 
added together. 
Card 2 for GENERALIZED stiffness option. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCIDPH 
LCIDT 
LCIDPS  DLCIDPH  DLCIDT  DLCIDPS 
Type 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none
Figure 10-30.  Definition of angles for the GENERALIZED joint stiffness. 
Card 3 for GENERALIZED stiffness option.  
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ESPH 
FMPH 
EST 
FMT 
ESPS 
FMPS 
Type 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Card 4 for GENERALIZED stiffness option. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSAPH 
PSAPH 
NSAT 
PSAT 
NSAPS 
PSAPS 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F
Case I: Elastic Perfectly Plastic Yield Curve
Case II: Load Curve Used for Yield Curve
friction
value
elastic
stiffness
load curve
Displacement
negative stop
displacement
Displacement
positive stop
displacement
negative stop
negative stop
displacement
displacement
positive stop
positive stop
displacement
displacement
Yield curve beyond stop angle
Yield curve
Example loading/unloading path
load curve
reflection
Figure 10-31.  Friction model.  The friction model is motivated by plasticity and
it is implemented for both rotational and translational joints.  In the context of
a  rotational  joint,  the  y-axis  is  to  be  interpreted  as  moment  (rotational  force)
and  the  x-axis  is  to  be  interpreted  as  rotation.    Case  I  (left)  is  activated  by  a 
positive friction value.  Case II (right) is activated by a negative integer friction
value, the absolute value of which specifies a load curve.  See the friction, elastic, 
and  stop  angle/displacement  parameters  from  the  input  cards  (FM[var],  ES[var], 
NSA[var], PSA[var]). 
  VARIABLE   
LCIDPH 
LCIDT 
LCIDPS 
DLCIDPH 
DLCIDT 
DESCRIPTION
Load  curve  ID  for  𝜙-moment  versus  rotation  in  radians.    See 
Figure 10-30.  If zero, the applied moment is set to 0.0.  See *DE-
FINE_CURVE. 
Load  curve  ID  for  𝜃-moment  versus  rotation  in  radians.    If  zero, 
the applied moment is set to 0.0.  See *DEFINE_CURVE. 
Load curve ID for 𝜓-moment versus rotation in radians.  If zero, 
the applied moment is set to 0.0.  See *DEFINE_CURVE.  
Load  curve  ID  for 𝜙-damping  moment  versus  rate  of  rotation  in 
radians  per  unit  time.    If  zero,  damping  is  not  considered.    See
*DEFINE_CURVE. 
Load  curve  ID  for  𝜃-damping  moment  versus  rate  of  rotation  in 
radians  per  unit  time.    If  zero,  damping  is  not  considered.    See
*DEFINE_CURVE.
VARIABLE   
DLCIDPS 
ESPH 
FMPH 
EST 
FMT 
ESPS 
FMPS 
DESCRIPTION
Load  curve  ID  for  𝜓-damping  torque  versus  rate  of  rotation  in 
radians  per  unit  time.    If  zero,  damping  is  not  considered.    See 
*DEFINE_CURVE. 
Elastic stiffness per unit radian for friction and stop angles  for 𝜙
rotation.    If  zero,  friction  and  stop  angles  are  inactive  for  𝜙
rotation. 
Frictional moment limiting value for 𝜙 rotation.  If zero, friction is 
inactive for 𝜙 rotation.  This option may also be thought of as an
elastic-plastic  spring.    If  a  negative  value  is  input  then  the
absolute value is taken as the load curve or table ID defining the
yield moment versus 𝜙 rotation.  A table permits the moment to 
also  be  a  function  of  the  joint  reaction  force  and  requires  the
specification of JID on card 1.  See Figure 10-31. 
Elastic  stiffness  per  unit  radian  for  friction  and  stop  angles  for  𝜃
rotation.      If  zero,  friction  and  stop  angles  are  inactive  for  𝜃
rotation.  See Figure 10-31. 
Frictional moment limiting value for 𝜃 rotation.  If zero, friction is 
inactive for 𝜃 rotation.  This option may also be thought of as an
elastic-plastic  spring.    If  a  negative  value  is  input  then  the
absolute value is taken as the load curve or table ID defining the
yield  moment  versus  𝜃  rotation.    A  table  permits  the  moment  to 
also  be  a  function  of  the  joint  reaction  force  and  requires  the
specification of JID on card 1. 
Elastic stiffness  per unit radian for friction and stop angles for 𝜓
rotation.    If  zero,  friction  and  stop  angles  are  inactive  for  𝜓
rotation. 
Frictional moment limiting value for 𝜓 rotation.  If zero, friction is 
inactive for 𝜓 rotation.  This option may also be thought of as an
elastic-plastic  spring.    If  a  negative  value  is  input  then  the
absolute value is taken as the load curve or table ID defining the
yield moment versus 𝜓 rotation.  A table permits the moment to 
also  be  a  function  of  the  joint  reaction  force  and  requires  the
specification of JID on card 1. 
NSAPH 
Stop angle in degrees for negative 𝜙 rotation.  Ignored if zero.  See 
Figure 10-31. 
PSAPH 
Stop angle in degrees for positive 𝜙 rotation.  Ignored if zero.
VARIABLE   
DESCRIPTION
NSAT 
PSAT 
Stop angle in degrees for negative 𝜃 rotation.  Ignored if zero. 
Stop angle in degrees for positive 𝜃 rotation.  Ignored if zero. 
NSAPS 
Stop angle in degrees for negative 𝜓 rotation.  Ignored if zero. 
PSAPS 
Stop angle in degrees for positive 𝜓 rotation.  Ignored if zero. 
Remarks: 
After the stop angles are reached the torques increase linearly to resist further angular 
motion  using  the  stiffness  values  on  Card  3.    Reasonable  stiffness  values  have  to  be 
chosen.  If the stiffness values are too low or zero, the stop will be violated. 
If  the  initial  local  coordinate  axes  do  not  coincide,  the  angles,  𝜙,  𝜃,  and    𝜓,  will  be 
initialized  and  torques  will  develop  instantaneously  based  on  the defined  moment  vs.  
rotation curves. 
There are two methods available to calculate the rotation angles between the coordinate 
systems.  For more information, see the JNTF parameter on *CONTROL_RIGID. 
Card 2 for TRANSLATIONAL stiffness option. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCIDX 
LCIDY 
LCIDZ 
DLCIDX 
DLCIDY 
DLCIDZ 
Type 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none
Card 3 TRANSLATIONAL stiffness option. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ESX 
FFX 
ESY 
FFY 
ESZ 
FFZ 
Type 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Card 4 for TRANSLATIONAL stiffness option. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSDX 
PSDX 
NSDY 
PSDY 
NSDZ 
PSDZ 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
  VARIABLE   
LCIDX 
LCIDY 
LCIDZ 
DLCIDX 
DESCRIPTION
Load curve ID for x-force versus x-distance between the origins of 
CIDA  and  CIDB  based  on  the  x-direction  of  CIDB.    If  zero,  the 
applied force is set to 0.0.  See *DEFINE_CURVE. 
Load curve ID for y-force versus y-distance between the origins of 
CIDA  and  CIDB  based  on  the  y-direction  of  CIDB.    If  zero,  the 
applied force is set to 0.0.  See *DEFINE_CURVE. 
Load curve ID for z-force versus z-distance between the origins of 
CIDA  and  CIDB  based  on  the  z-direction  of  CIDB.    If  zero,  the 
applied force is set to 0.0.  See *DEFINE_CURVE. 
Load  curve  ID  for  x-damping  force  versus  rate  of  x-translational 
displacement  per  unit  time  between  the  origins  of  CIDA  and
CIDB  based  on  the  x-direction  of  CIDB.    If  zero,  damping  is  not 
considered.  See *DEFINE_CURVE.
VARIABLE   
DLCIDY 
DLCIDZ 
ESX 
FFX 
ESY 
FFY 
ESZ 
FMZ 
DESCRIPTION
Load  curve  ID  for  y-damping  force  versus  rate  of  y-translational 
displacement  per  unit  time  between  the  origins  of  CIDA  and
CIDB  based  on  the  y-direction  of  CIDB.    If  zero,  damping  is  not 
considered.  See *DEFINE_CURVE. 
Load  curve  ID  for  z-damping  force  versus  rate  of  z-translational 
displacement  per  unit  time  between  the  origins  of  CIDA  and
CIDB  based  on  the  z-direction  of  CIDB.    If  zero,  damping  is  not 
considered.  See *DEFINE_CURVE. 
Elastic  stiffness  for  friction  and  stop  displacement  for  x-
translation.    If  zero,  friction  and  stop  angles  are  inactive  for  x-
translation.  See Figure 10-31. 
Frictional force limiting value for x-translation.  If zero, friction is 
inactive for x-translation.  This option may  also be thought of as
an  elastic-plastic  spring.    If  a  negative  value  is  input  then  the
absolute  value  is  taken  as  the  load  curve  ID  defining  the  yield
force versus x-translation.  See Figure 10-31. 
Elastic  stiffness  for  friction  and  stop  displacement  for  y-
translation.      If  zero,  friction  and  stop  angles  are  inactive  for  y-
translation. 
Frictional force limiting value for y-translation.  If zero, friction is 
inactive for y-translation.  This option may also be thought of as
an  elastic-plastic  spring.    If  a  negative  value  is  input  then  the
absolute  value  is  taken  as  the  load  curve  ID  defining  the  yield
force versus y-translation. 
Elastic  stiffness  for  friction  and  stop  displacement  for  z-
translation.    If  zero,  friction  and  stop  angles  are  inactive  for  z-
translation. 
Frictional force limiting value for z-translation.  If zero, friction is 
inactive  for  z-translation.    This  option  may  also  be  thought  of  as 
an  elastic-plastic  spring.    If  a  negative  value  is  input  then  the
absolute  value  is  taken  as  the  load  curve  ID  defining  the  yield
force versus z-translation. 
NSDX 
Stop displacement for negative x-translation.  Ignored if zero.  See 
Figure 10-31. 
PSDX 
Stop displacement for positive x-translation.  Ignored if zero.
VARIABLE   
DESCRIPTION
Stop displacement for negative y-translation.  Ignored if zero. 
Stop displacement for positive y-translation.  Ignored if zero. 
Stop displacement for negative z-translation.  Ignored if zero. 
Stop displacement for positive z-translation.  Ignored if zero. 
NSDY 
PSDY 
NSDZ 
PSDZ 
Remarks: 
After  the  stop  displacements  are  reached  the  force  increases  linearly  to  resist  further 
translational  motion  using  the  stiffness  values  on  Card  3.    Reasonable  stiffness  values 
must be chosen.  If the stiffness values are too low or zero, the stop will be violated. 
Example: 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *CONSTRAINED_JOINT_STIFFNESS_GENERALIZED 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Define a joint stiffness for the revolute joint described in  
$    *CONSTRAINED_JOINT_REVOLUTE 
$ 
$  Attributes of the joint stiffness: 
$    - Used for defining a stop angle of 30 degrees rotation 
$        (i.e., the joint allows a positive rotation of 30 degrees and 
$           then imparts an elastic stiffness to prevent further rotation) 
$    - Define between rigid body A (part 1) and rigid body B (part 2) 
$    - Define a local coordinate system such that local x corresponds 
$         to the joint’s axis of revolution and the angle phi is the angle 
$         of rotation about that axis. 
$    - The elastic stiffness per unit radian for the stop angle is 100. 
$    - Variables left blank are not used during the simulation. 
$ 
*CONSTRAINED_JOINT_STIFFNESS_GENERALIZED 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$     jsid      pida      pidb      cida      cidb 
         1         1         2         5         5 
$ 
$   lcidph     lcidt    lcidps   dlcidph    dlcidt   dlcidps 
$ 
$     esph      fmps       est       fmt      esps      fmps 
     100.0                
$ 
$    nsaph     psaph      nsat      psat     nsaps     psaps 
                30.0 
$ 
$ 
*DEFINE_COORDINATE_NODES 
$      cid        n1        n2        n3
5         1         2         3 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$
*CONSTRAINED_JOINT_USER_FORCE 
Purpose:    Define  input  data  for  a  user  subroutine  to  generate  force  resultants  as  a 
function of time and joint motion. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FID 
JID 
NHISV 
Type 
I 
I 
Default 
none 
none 
I 
0 
User Subroutine Constants Cards.  Define up to 48 optional user constants  (6 cards 
total)  for the user subroutine.  This input is terminated after 48 constants are defined 
or when the next “*” keyword card is encountered.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CONST1  CONST2  CONST3  CONST4  CONST5  CONST6  CONST7  CONST8 
Type 
F 
F 
F 
F 
F 
I 
I 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
FID 
JID 
NHISV 
Joint user force ID. 
Joint ID for which this user force input applies. 
Number of history variables required for this definition.  An array
NHISV  long  is  allocated  and  passed  into  the  user  subroutine.
This array is updated in the user subroutine. 
CONSTn 
A constant which is passed into the user subroutine.
*CONSTRAINED_LAGRANGE_IN_SOLID_{OPTION1}_{OPTION2} 
Purpose:    This  command  provides  the  coupling  mechanism  for  modeling  Fluid-
Structure  Interaction  (FSI).    The  structure  can  be  constructed  from  Lagrangian  shell 
and/or solid entities.  The multi-material fluids are modeled by ALE formulation. 
Available options for OPTION1 include: 
<BLANK> 
EDGE 
This option may be used to allow the coupling between the edge of a shell part or part 
set  and  one  or  more  ALE  multi-material  groups  (AMMG).    It  accounts  for  the  shell 
thickness  in  the  coupling  calculation.    The  edge  thickness  is  the  same  as  the  shell 
thickness.  This option only works when the Lagrangian slave set is defined as a part or 
a part set ID.  It will not work for a slave segment set.  One application of this option is a 
simulation of a Lagrangian blade (a shell part) cutting through some ALE material. 
Available options for OPTION2 include: 
<BLANK> 
TITLE 
To define a coupling (card) ID number and title for each coupling card.  If a title is not 
defined LS-DYNA will automatically create an internal title for this coupling definition.  
The  ID  number  can  be  used  to  delete  coupling  action  in  a  restart  input  deck  via  the 
*DELETE_FSI card. 
Title Card.  Additional card for the TITLE keyword option. 
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
COUPID 
Type 
I 
TITLE 
A70
Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SLAVE  MASTER 
SSTYP 
MSTYP 
NQUAD 
CTYPE 
DIREC 
MCOUP 
Type 
I 
I 
Default 
none 
none 
  Card 2 
1 
2 
I 
0 
3 
I 
0 
4 
I 
0 
5 
I 
2 
6 
I 
1 
7 
I 
0 
8 
Variable 
START 
END 
PFAC 
FRIC 
FRCMIN 
NORM  NORMTYP  DAMP 
Type 
Default 
  Card 3 
Variable 
Type 
F 
0 
1 
K 
F 
F 
F 
F 
F 
1.0E10 
0.1 
0.0 
0.5 
2 
3 
4 
5 
I 
0 
6 
I 
0 
7 
F 
0.0 
8 
HMIN 
HMAX 
ILEAK 
PLEAK 
LCIDPOR 
NVENT 
IBLOCK 
Default 
0.0 
none 
none 
F 
F 
I 
0 
F 
0.1 
I 
0 
I 
0 
I 
0 
Card 4a.   This card is required for CTYPE 11 & 12 but is otherwise optional.  
  Card 4a 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IBOXID 
IPENCHK 
INTFORC 
IALESOF 
LAGMUL  PFACMM 
THKF 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
F 
0.0 
I 
0 
F 
0.0
Porous Coupling Card 4b.  This card applies only to CTYPE 11 & 12.  If 4b is defined, 
4a must be defined before 4b. 
  Card 4b 
Variable 
1 
A1 
Type 
F 
2 
B1 
F 
3 
A2 
F 
4 
B2 
F 
5 
A3 
F 
6 
B3 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
7 
8 
POREINI 
F 
0.0 
Venting  Geometry  Card(s)  4c.    These  card(s)  set  venting  geometry.    It  is  repeated 
NVENT times (one card for defining each vent hole).  It is defined only if NVENT > 0 in 
card 3.  The last NVENT cards for *CONSTRAINED_LAGRANGE_IN_SOLID are taken 
to  be  Card(s)  4c,  therefore,  Cards  4a  and  4b  are  not  mandatory  when  Card(s)  4c  are 
defined.   
  Card 4c 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VENTSID 
VENTYP 
VTCOEF  POPPRES
COEFLC 
Type 
Default 
I 
0 
I 
0 
I 
0 
F 
0.0 
I 
0 
  VARIABLE   
COUPID 
DESCRIPTION
Coupling (card) ID number.  This ID can be used in a restart input
deck  to  delete  or  reactivate  this  coupling  action  via  the
*DELETE_FSI  card.    If  not  defined,  LSDYNA  will  assign  an 
internal  coupling  ID  based  on  the  order  of  appearance  in  the
input deck. 
TITLE 
A description of this coupling definition (A70). 
SLAVE 
Slave  set  ID  defining  a  part,  part  set  or  segment  set  ID  of  the 
Lagrangian or slave structure .  See Remark 1. 
MASTER 
Master set ID defining a part or part set ID of the ALE or master 
solid elements .
VARIABLE   
DESCRIPTION
SSTYP 
Slave set type of “SLAVE” : 
EQ.0:  part set ID (PSID). 
EQ.1:  part ID (PID). 
EQ.2:  segment set ID (SGSID). 
MSTYP 
Master set type of “MASTER” : 
EQ.0:  part set ID (PSID). 
EQ.1:  part ID (PID). 
NQUAD 
Number  of  coupling  points  distributed  over  each  coupled
Lagrangian surface segment.   
EQ.0:  NQUAD will be set by default to 2, 
GT.0:  An  NQUAD  ×  NQUAD  coupling  points  distribution
over each Lagrangian segment is defined, 
LT.0:  NQUAD is reset to a positive value.  Coupling at nodes 
is obsolete. 
CTYPE 
Fluid-Structure  coupling  method.    The  constraint  methods  (1,  2,
and 3) are not supported in MPP. 
EQ.1:  constrained acceleration. 
EQ.2:  constrained  acceleration  and  velocity  (default,  see
Remark 3). 
EQ.3:  constrained acceleration and velocity, normal direction
only. 
EQ.4:  penalty coupling for shell (with or without erosion) and
solid elements (without erosion). 
NOTE:  For  RIGID  slave  PARTS  a  penalty  cou-
pling method (CTYPE=4) must be used, 
see parameter CTYPE below. 
EQ.5:  penalty  coupling  allowing  erosion  in  the  Lagrangian
entities (solid elements and thick shells). 
EQ.6:  penalty  coupling  designed  for  airbag  modeling  which
automatically controls the DIREC parameter internally. 
It  is  equivalent  to  setting  {CTYPE = 4;  DIREC = 1}  for 
unfolded  region;  and  {CTYPE = 4;  DIREC = 2};  in  fold-
VARIABLE   
DESCRIPTION
ed region.  For both cases: {ILEAK = 2; FRCMIN = 0.3}.
EQ.11:  coupling designed to couple Lagrangian porous shell to
ALE material.  When this option is used, THKF, the 7th
column  parameter  of  optional  card  4a  and  the  first  2
parameters  of  optional  card  4b  must  be  defined.    See
*LOAD_BODY_POROUS and remark 13 below. 
EQ.12:  coupling  designed  to  couple  Lagrangian  porous  solid 
to ALE material.  When this option is used, Ai & Bi pa-
rameters  of  optional  card  4b  must  be  defined  (card  4a
must  be  defined  but  can  be  blank).    See  *LOAD_-
BODY_POROUS and Remark 14 below 
DIREC 
For CTYPE=4, 5, or 6 
Coupling direction:  
EQ.1:  normal direction, compression and tension (default) 
EQ.2:  normal direction, compression only 
EQ.3:  all directions 
For CTYPE=12 
Flag to activate an element coordinate system: 
EQ.0:  The forces are applied in the global directions. 
EQ.1:  The  forces  are  applied  in  a  local  system  attached  to  the
Lagrangian  solid. 
is  consistent  with
  The  system 
AOPT = 1 in *LOAD_BODY_POROUS.  .
MCOUP 
For CTYPE = 4, 5, 6, 11, or 12 
Multi-material option:   
EQ.0:  couple with all multi-material groups, 
EQ.1:  couple with material with highest density. 
LT.0:  MCOUP must be an integer.  -MCOUP refers to a set ID 
of an ALE multi-material group.  See *SET_MULTI-MA-
TERIAL_GROUP. 
START 
Start time for coupling. 
END 
End time for coupling.  If less than zero, coupling will be turned
off during dynamic relaxation.  After dynamic relaxation phase is
finished, the absolute value will be taken as end time.
VARIABLE   
PFAC 
DESCRIPTION
For CTYPE = 4,5 or 6 
Penalty  factor.    PFAC  is  a  scale  factor  for  scaling  the  estimated 
stiffness  of  the  interacting  (coupling)  system.    It  is  used  to
compute  the  coupling  forces  to  be  distributed  on  the  slave  and
master parts 
GT.0:  Fraction of estimated critical stiffness. 
LT.0:  PFAC  must be an integer, and -PFAC is a load curve ID. 
The curve defines the coupling pressure on the y-axis as 
a function of the penetration along the x-axis.   
For CTYPE = 11 or 12 
Time step factor 
FRIC 
Coefficient of friction (used with DIREC = 1 and 2 only). 
FRCMIN 
Minimum  volume  fraction  of  a  coupled  ALE  multi-material 
group  (AMMG)  or  fluid  in  a  multi-material  ALE  element  to 
activate  coupling.    Default  value  is  0.5.    Reducing  FRCMIN
(typically, between 0.1 and 0.3) would turn on coupling earlier to 
prevent leakage in high velocity impact cases. 
NORM 
A Lagrangian segment will couple to fluid on only one side of the
segment.  NORM determines which side.  See Remark 6. 
EQ.0:  Couple  to  fluid  (AMMG)  on  head-side  of  Lagrangian 
segment normal vector. 
EQ.1:  Couple  to  fluid  (AMMG)  on  tail-side  of  Lagrangian 
segment normal vector. 
NORMTYP 
Penalty coupling spring (or force) direction (DIREC = 1, or 2): 
EQ.0:  normal  vectors  are  interpolated  from  nodal  normals. 
(default). 
EQ.1:  normal  vectors  are  interpolated  from  segment  normals.
This is  sometimes a little more robust for sharp Lagran-
gian corners, and folds. 
DAMP 
Damping factor for penalty coupling.  This is a coupling-damping 
scaling factor.  Typically it may be between 0 and 1 .
VARIABLE   
DESCRIPTION
K 
HMIN 
Thermal conductivity of a virtual fluid between the slave surface
and the master material  . 
The absolute value is minimum air gap in heat transfer, ℎmin . 
LT.0:  turn  on  constraint  based  thermal  nodal  coupling
between LAG structure and ALE fluids. 
GE.0:  minimum air gap.  If zero, default to 1.0e-6. 
HMAX 
Maximum air gap in heat transfer, ℎmax.  There is no heat transfer 
above this value . 
ILEAK 
Coupling leakage control flag (Remark 9): 
EQ.0:  none (default), 
EQ.1:  weak, leakage control is turned off if  
penetrating volume fraction > FRCMIN + 0.2 
EQ.2:  strong,  with  improved  energy  consideration.    Leakage
control is turned off if  
penetrating volume fraction > FRCMIN + 0.4
PLEAK 
Leakage control penalty factor, 0 < PLEAK < 0.2 is recommended. 
This factor influences the additional coupling force magnitude to
prevent  leakage.    It  is  conceptually  similar  to  PFAC.    Almost
always, the default value (0.1) is adequate. 
LCIDPOR 
If  this  is  a  positive  integer:    A  load  curve  ID  (LCID)  defining 
porous flow through coupling segment: 
Abscissa = 𝑥 = (𝑃up − 𝑃down) 
Ordinate = 𝑦 = relative porous fluid velocity 
Where  Pup  and  Pdown  are,  respectively,  the  upstream  and 
downstream  pressures  across  of  the  porous  coupling  segment.
The  relative  porous  velocity  is  the  ALE  fluid  velocity  relative  to
the  moving  Lagrangian  segment.    This  experimental  data  curve
must be provided by the user. 
If LCIDPOR is a negative integer:  The porous flow is  controlled
by the parameters FLC, FAC, ELA under *MAT_FABRIC card.
VARIABLE   
DESCRIPTION
CAUTION:  The  pressure  under  the  FAC  load  curve  is 
“absolute  upstream  pressure”  . 
Abscissa = 𝑥 = absolute upstream pressure 
Ordinate = 𝑦 = relative porous fluid velocity 
For CTYPE = 11 or CTYPE = 12 and POREINI = 0.0: 
LT.0:  The load curve |LCIDPOR| is a factor versus time of the
porous  force  computed  by  the  Ergun  equation  . 
GT.0:  The  load  curve  LCIDPOR  is  a  porous  force  versus
velocity,  which  replaces  the  force  computed  by  the
Ergun equation . 
For CTYPE = 11 or CTYPE = 12 and POREINI > 0.0: 
NE.0:  The load curve |LCIDPOR| is a factor versus time of the
porous  force  computed  by  the  Ergun  equation  . 
The  number  of  vent  surface  areas  to  be  defined.    Each  venting
flow surface is represented by one or more Lagrangian segments
(or surfaces). 
For  airbag  applications,  this  may  be  referred  to  as  “isentropic”
venting  where  the  isentropic  flow  equation  is  used  to  compute
the  mass  flow  rate  based  on  the  ratio  of  the  upstream  and
downstream pressures 𝑃up/𝑃down. 
For  each  of  the  NVENT  vent  surfaces,  an  additional  card  of
format  4c  defining  the  geometrical  and  flow  properties  for  each
vent surface will be read in. 
The  vented  mass  will  simply  be  deleted  from  the  system  and
cannot  be  visualized  as  in  the  case  of  physical  venting  . 
NVENT
VARIABLE   
IBLOCK 
DESCRIPTION
Flag  to  control  the  venting  (or  porous)  flow  blockage  due  to
Lagrangian contact during ALE computation. 
EQ.0:  Off 
EQ.1:  On 
The venting definition is defined in this command.  However, the
venting  flow  may  be  defined  via  either  the  LCIDPOR  parameter 
in  this  command  or  via  the  *MAT_FABRIC  parameters  (FLC, 
FAC,  ELA).    However,  note  that  FVOPT  (blocking)  parameter 
under *MAT_FABRIC applies only to CV computation. 
IBOXID 
A box ID defining a box region in space in which ALE coupling is
activated. 
GT.0:  At  time = 0.0,  the  Lagrangian  segments  inside  this  box
are  remembered.    In  subsequent  coupling  computation 
steps, there is no need to search for the Lagrangian seg-
ments again. 
LT.0:  At  each  FSI  bucketsort,  the  Lagrangian  segments  inside
this  box  are  marked  as  active  coupling  segments.    This
makes the coupling operate more efficiently when struc-
ture  mesh  is  approaching  ALE  domain,  i.e.    hydroplan-
ing, bird strike, etc.  
IPENCHK 
Only for CTYPE = 4 
Initial penetration check flag : 
EQ.0:  Do not check for initial penetration. 
EQ.1:  Check and save initial ALE material penetration across a 
Lagrangian  surface  (d0),  but do  not  activate  coupling  at
t = 0.  In subsequent steps (t > 0) the actual penetration is 
computed as follows: 
Actual Penetration
⏟⏟⏟⏟⏟⏟⏟⏟⏟
𝑑𝑎
= Total Penetration
⏟⏟⏟⏟⏟⏟⏟⏟⏟
𝑑𝑇
− Initial Penetration
⏟⏟⏟⏟⏟⏟⏟⏟⏟
𝑑0
INTFORC 
A flag to turn on or off the output of ALE coupling pressure and
forces on the slave Lagrangian segments (or surfaces). 
EQ.0:  Off 
EQ.1:  On 
Note that the coupling pressures and forces are computed based
VARIABLE   
DESCRIPTION
on the coupling stiffness reponse to the ALE fluid penetration. 
When  INFORC = 1  and  a  *DATABASE_BINARY_FSIFOR  (DBF) 
card  is  defined,  LS-DYNA  writes  out  the  segment  coupling 
pressure  and  forces  to  the  binary  interface  force  file  for  contour
plotting.    This  interface  force  file  must  be  given  a  name  on  the 
execution line, for example: 
ls-dyna  i=inputfilename.k … h=interfaceforcefilename 
The  time  interval  between  output  is  defined  by  “dt”  in  the  DBF 
card.  To plot the binary data in this file: 
ls-prepost interfaceforcefilename 
IALESOF 
An  integer  flag  to  turn  ON/OFF  a  supplemental  Lagrange
multiplier  FSI  constraint  which  provides  a  coupling  force  in
addition  to  the  basic  penalty  coupling  contribution.    This  is  a
hybrid coupling method. 
EQ.0:  OFF (default). 
EQ.1:  Turn  ON  the  hybrid  Lagrange-multiplier  method. 
LAGMUL multiplier factor is read. 
LAGMUL 
A  Lagrange  multiplier  factor  with  a  range  between  0.0  and  0.05
may be defined.  A typical value may be 0.01.  This should never
be greater than 0.1.  
EQ.0:  OFF (default). 
GT.0:  Turn  ON  the  Lagrange-multiplier  method  and  use 
LAGMUL as a coefficient for scaling the penalty factor. 
PFACMM 
Mass-based  penalty  stiffness  factor  computational  options.    This
works  in  conjunction  with  PFAC = constant  (not  a  load  curve). 
The  coupling  penalty  stiffness  (CPS)  is  computed  based  on  an 
estimated effective coupling mass.   
EQ.0:  CPS  ∝ PFAC × min (𝑚slave, 𝑚master) , default. 
EQ.1:  CPS ∝ PFAC × max (𝑚slave, 𝑚master) . 
EQ.2:  CPS ∝ PFAC × √𝑚slave𝑚master  ,  geometric-mean  of  the 
masses. 
EQ.3:  CPS ∝ PFAC × 𝐾Lagrangian  where  K  is  the  bulk  modulus 
of the slave or Lagrangian part
VARIABLE   
THKF 
DESCRIPTION
For all CTYPE choices except 11: 
A  flag  to  account  for  the  coupling  thickness  of  the  Lagrangian
shell (slave) part.   
LT.0:  Use  positive  value  of  |THKF|  for  coupling  segment
thickness. 
EQ.0:  Do not consider coupling segment thickness. 
GT.0:  Coupling segment thickness scale factor. 
For CTYPE = 11: 
This thickness is required for volume calculation. 
GT.0:  (Fabric)  Thickness  scale  factor.    The  base  shell  thickness
is taken from the *PART definition. 
LT.0:  User-defined  (Fabric)  thickness.    The  fabric  thickness  is
set to |THKF|. 
A1 
Viscous  coefficient  for  the  porous  flow  Ergun  equation  . 
GT.0:   
For CTYPE = 11 
which is the coefficient for normal-to-segment direction. 
A1 = 𝐴𝑛 
For CTYPE = 12 
A1 = 𝐴𝑥 
which  is  the  coefficient  for  the  x-direction  in  the 
coordinate system specified by DIREC. 
LT.0:  If  POREINI = 0.0,  the  coefficient  is  time  dependent 
through  a  load  curve  id  defined  by  |A1|.    If  POREI-
NI > 0.0,  the  coefficient  is  porosity  dependent  through a
load curve id defined by |A1|.  The porosity is defined
by PORE . 
B1 
Inertial  coefficient  for  the  porous  flow  Ergun  equation  . 
GT.0:   
For CTYPE = 11 
B1 = 𝐵𝑛
VARIABLE   
DESCRIPTION
A2 
B2 
which is the coefficient for normal-to-segment direction. 
For CTYPE = 12 
B1 = 𝐵𝑥 
which is the coefficient for the x-direction of a coordinate 
system specified by DIREC. 
LT.0:  If  POREINI = 0.0,  the  coefficient  is  time  dependent 
through  a  load  curve  id  defined  by  |B1|.    If  POREI-
NI > 0.0,  the  coefficient  is  porosity  dependent  through a
load  curve  id  defined  by  |B1|.    The  porosity  is  defined
by PORE . 
For CTYPE = 12 
Viscous  coefficient  for  the  porous  flow  Ergun  equation  . 
GT.0:  Coefficient  for  the  y-direction  of  a  coordinate  systems 
specified by DIREC. 
A2 = 𝐴𝑦 
LT.0:  If  POREINI = 0.0,  the  coefficient  is  time  dependent 
through  a  load  curve  id  defined  by  |A1|.    If  POREI-
NI > 0.0,  the  coefficient  is  porosity  dependent  through a
load curve id defined by |A2|.  The porosity is defined
by PORE . 
For CTYPE=12 
Inertial  coefficient  for  the  porous  flow  Ergun  equation  . 
GT.0: Coefficient  for  the  y-direction  of  a  coordinate  system 
specified by DIREC. 
B2 = 𝐵𝑦 
LT.0:  If  POREINI = 0.0  and  B2 < 0,  the  coefficient  is  time 
dependent  through  a  load  curve  id  defined  by  |B2|.    If
POREINI > 0.0  and  B2 < 0,  the  coefficient  is  porosity 
dependent through a load curve id defined by |B2|.  The
porosity is defined by PORE . 
A3 
For CTYPE = 12 
Viscous  coefficient  for  the  porous  flow  Ergun  equation  .
VARIABLE   
DESCRIPTION
GT.0:  Coefficient  for  the  z-direction  of  a  coordinate  system 
specified by DIREC. 
A3 = 𝐴𝑧 
LT.0:  If  POREINI = 0.0  and  A3 < 0,  the  coefficient  is  time 
dependent through a load curve id defined by |A3|.  If
POREINI > 0.0  and  A3 < 0,  the  coefficient  is  porosity 
dependent  through  a  load  curve  id  defined  by  |A3|.
The porosity is defined by PORE . 
B3 
For CTYPE = 12 
Inertial  coefficient  for  the  porous  flow  Ergun  equation  . 
GT.0:  Coefficient  for  the  z-direction  of  a  coordinate  system 
specified by DIREC. 
B3 = 𝐵𝑧 
LT.0:  If  POREINI = 0.0  and  B3 < 0,  the  coefficient  is  time 
dependent  through  a  load  curve  id  defined  by  |B3|.    If
POREINI > 0.0  and  B3 < 0,  the  coefficient  is  porosity 
dependent  through  a  load  curve  id  defined  by  |B3|.
The porosity is defined by PORE . 
POREINI 
For CTYPE = 11 or CTYPE = 12 
POREINI is the initial volume of pores in an element.  The current
volume is 
PORE = POREINI ×
𝑣(𝑡)
𝑣(𝑡0)
where 𝑣(𝑡) and  𝑣(𝑡0) are the current and initial element volumes 
respectively. 
VENTSID 
Set ID of the vent hole shape. 
VENTYP 
Vent surface area set ID type: 
EQ.0:  Part set ID (PSID). 
EQ.1:  Part ID (PID). 
EQ.2:  Segment set ID (SGSID). 
VTCOEF 
Flow coefficient for each vent surface area.
VARIABLE   
POPPRES 
DESCRIPTION
Venting  pop  pressure  limit.    If  the  pressure  inside  the  airbag  is
lower than this pressure, then nothing is vented.  Only when the 
pressure  inside  the  airbag  is  greater  than  POPPRES  that  venting
can begin. 
COEFLC 
A  time-dependent  multiplier  load  curve  for  correcting  the  vent
flow coefficient, with values ranging from 0.0 to 1.0. 
Best Practices: 
Due  to  the  complexity  of  this  card,  some  comments  on  simple,  efficient  and  robust 
coupling  approach  are  given  here.    These  are  not  rigid  guidelines,  but  simply  some 
experience-based observations. 
1.  Definition  (Fluid  and  Structure).    The  term  fluid,  in  the  Fluid-Structure 
Interaction (FSI), refers to materials with ALE element formulation, not indicat-
ing the phase (solid, liquid or gas) of those materials.  In fact, solid, liquid and 
gas  can  all  be  modeled  by  the  ALE  formulation.    The  term  structure  refers  to 
materials with Lagrangian element formulation. 
2.  Default Values (CTYPE and MCOUP).  In general, penalty coupling (CTYPE 4 
& 5) is recommended, and MCOUP=negative integer is a better choice to define 
a specific ALE multi-material group (AMMG) to be coupled to the Lagrangian 
surface.  At the minimum, all parameters on card 1 are to be specified, and the 
default values for most are good starting choices (except MCOUP). 
3.  How  to  Correct  Leakage.    If  there  is  leakage,  PFAC,  FRCMIN,  NORMTYPE 
and ILEAK are the 4 parameters that can be adjusted. 
a)  For hard structure (steel) and very compressible fluid (air), PFAC may be 
set to 0.1 (or higher).  PFAC = constant value. 
b)  Next,  keeping  PFAC = constant  and  set  PFACMM = 3  (optional  card  4a).  
This option scales the penalty factor by the bulk modulus of the Lagrangi-
an structure.  This new approach has also shown to be effective for some 
airbag application. 
c)  The next approach may be switching from constant PFAC to a load curve 
approach (i.e.  PFAC = load curve, and PFACMM = 0).  By looking at the 
pressure in the system near leakage original location, we can get a feel for 
the pressure required to stop it.
d)  If leakage persists after some iterations on the coupling force controls, one 
can subsequently try to set ILEAK = 2 in combination with the other con-
trols to prevent leakage. 
e)  If the modifications fail to stop the leakage, maybe the meshes have to be 
redesigned  to  allow  better  interactions  between  the  Lagrangian  and  Ale 
materials. 
In the example below, the underlined parameters are usually defined parame-
ters.  A full card definition is shown for reference. 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
*CONSTRAINED_LAGRANGE_IN_SOLID 
$    SLAVE    MASTER     SSTYP     MSTYP     NQUAD     CTYPE     DIREC     MCOUP 
         1        11         0         0         4         4         2      -123 
$    START       END      PFAC      FRIC    FRCMIN      NORM  NORMTYPE      DAMP 
       0.0       0.0       0.1      0.00       0.3         0         0       0.0 
$       CQ      HMIN      HMAX     ILEAK     PLEAK   LCIDPOR     NVENT    IBLOCK 
         0         0         0         0       0.0         0         0         0 
$4A IBOXID   IPENCHK   INTFORC   IALESOF    LAGMUL    PFACMM      THKF 
$        0         0         0         0         0         0         0  
$4B     A1        B1        A2        B2        A3        B3 
$      0.0       0.0       0.0       0.0       0.0       0.0 
$4C VNTSID   VENTYPE  VENTCOEF   POPPRES  COEFLCID  (STYPE:0=PSID;1=PID;2=SGSID) 
$        0         0         0       0.0         0  
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 
Remarks: 
1.  Meshing.  In order for a fluid-structure interaction (FSI) to occur, a Lagrangian 
(structure or slave) mesh must spatially overlap with an ALE (fluid or master) 
mesh.    Each  mesh  should  be  defined  with  independent  node  IDs.    LS-DYNA 
searches for the spatial intersection of between the Lagrangian and ALE mesh-
es.  Where the meshes overlap, there is a possibility that interaction may occur.  
In general, SLAVE, MASTER, SSTYP and MSTYPE are required definitions for 
specifying overlapping-domains coupling search. 
2.  Number  of  Coupling  Points.    The  number  of  coupling  points,  NQUAD  × 
NQUAD, is distributed over the surface of each Lagrangian segment.  General-
ly,  2  or  3  coupling  points  per  each  Eulerian/ALE  element  width  is  adequate.  
Consequently, the appropriate NQUAD values must be estimated based on the 
relative resolutions between the Lagrangian and ALE meshes. 
For  example,  if  1  Lagrangian  shell  element  spans  2  ALE  elements,  Then 
NQUAD for each Lagrangian segment should be 4 or 6.  Alternatively, if 2 or 3 
Lagrangian segments span 1 ALE element, then maybe NQUAD = 1 would be 
adequate. 
If  either  mesh  compresses  or  expands  during  the  interaction,  the  number  of 
coupling points per ALE element will also change.  The user must account for 
this  and  try  to  maintain  at  least  2  coupling  points  per  each  ALE  element  side
length during the whole process to prevent leakage.  Too many coupling points 
can result in instability, and not enough can result in leakage. 
3.  The  Constraint  Method.    The  constraint  method  violates  kinetic  energy 
balance. 
  The  penalty  method  is  therefore  recommended.  Historically, 
CTYPE=2  was  sometimes  used  to  couple  Lagrangian  beam  nodes  to  ALE  or 
Lagrangian solids, e.g., for modeling rebar in concrete, or tire cords in rubber.  
solids, 
For 
*CONSTRAINED_BEAM_IN_SOLID is now preferred. 
constraint-based 
coupling 
beams 
such 
in 
of 
4.  Coupling  Direction.    DIREC=2  (compression  only)  may  be  generally  a  more 
stable  and  robust  choice  for  coupling  direction.    However,  the  physics  of  the 
problem  should  dictate  the  coupling  direction.    DIREC=1  couples  under  both 
tension and compression.  This is sometimes useful; for example, in the case of a 
suddenly  accelerating  liquid  in  a  container.    DIREC=3  is  rarely  appropriate 
because it models an extremely sticky fluid. 
5.  Multi-material  Coupling  Option.    When  MCOUP  is  a  negative  integer;  for 
example  MCOUP=  -123,  then  an  ALE  multi-material  set-ID  (AMMSID)  of  123 
must exist.  This is an ID defined by a *SET_MULTI-MATERIAL_GROUP_LIST 
card.  This generally seems to be a better approach to couple to a specific set of 
AMMGs, and have a clearly defined fluid interface interacting with a Lagrangi-
an surface.  That way, any leakage may be visualized and the penalty force can 
be computed more precisely. 
The  Couple  to  all  materials  option  as  activated  by  MCOUP =  0  is  generally  not 
recommended.  LS-DYNA calculates the fluid coupling interface as the surface 
where the sum of coupled ALE materials occupies a volume fraction (Vf) equal 
to 50%.  Since MCOUP = 0 couples to all materials, the sum of all coupled ALE 
materials is, in this case, trivially 100%.  Consequently, when MCOUP = 0 there 
will not be a fluid interface with which to track leakage.
Shell
Shell normal vector
Shell normal vector
Fluid
Fluid & Shell
will interact
Shell Motion
Void
Shell Motion
Fluid
Shell
Void
Fluid & Shell will
not interact, use
NORM = 1 to
reverse the vector
Shell normal vector
Shell normal vector
Figure 10-32.  Shell Motion 
6.  Normal Vector Direction.  The normal vectors (NV) of a Lagrangian shell part 
are  defined  by  the  order  of  the  nodes  in  *ELEMENT  definitions,  via  the  right 
hand  rule,  and  for  a  segment  set,  the  order  of  nodes  defined  in  *SET_SEG-
MENT.    Let  the  side  pointed  to  by  NV  be  “positive”.    The  penalty  method 
measure penetration as the distance the ALE fluid penetrates from the positive 
side to the negative side of the Lagrangian segment.  Only fluid on the positive 
side will be “seen” and coupled to. 
Therefore, all normal vectors of the Lagrangian segments should point uniform-
ly toward the ALE fluid(s), AMMGs, to be coupled to.  If NV point uniformly 
away  from  the  fluid,  coupling  is  not  activated.    In  this  case,  coupling  can  be 
activated  by  setting  NORM = 1.    Sometimes  a  shell  part  or  mesh  is  generated 
such that its normal vectors do not point uniformly in a consistent direction (all 
toward the inside or outside of a container, etc.)  The user should always check 
for the normal vectors of any Lagrangian shell part interacting with any fluid.  
The NORM parameter may be used to flip the normal direction of all the seg-
ments included in the Lagrangian slave set.  See Figure 10-32. 
7.  Coupling-Damping Factor.  The user-input coupling-damping factor (DAMP) 
is used to scale down the critical-damping force (~ damper constant × velocity).  
For  a  mass-to-rigid-wall  system  connected  by  a  parallel-spring-damper  con-
nector,  we  can  obtain  solution  for  a  critically-damped  case.    DAMP  is  a  factor 
for  scaling  down  the  amount  of  damping,  with  DAMP=1  being  a  critically-
damped case.
8.  Heat  Transfer.    The  method  used  is  similar  to  that  done  by  *CONTACT_…_
THERMAL_… card, except radiation heat transfer is not considered.  A gap, 𝑙, 
is  assumed  to  exist  between  the  2  materials  undergoing  heat  transfer  (one  is 
Lagrangian and the other ALE).  The convection heat transfer in the gap is as-
sumed to approach simple conduction across the medium in the gap. 
𝑞 = 𝐾
𝑑𝑇
𝑑𝑥
~ℎΔ𝑇 ⇒ ℎ~
The  heat  flux  is  typically  defined  as  an  energy  transfer  rate  per  unit  area, 
𝑞 ∼ [ 𝐽 𝑠 ⁄ ]
𝑚2 .  The constant K is the thermal conductivity of the material in the gap; 
ℎ, is the equivalent convection heat transfer coefficient; and Δ𝑇 is the tempera-
ture difference between the master and slave sides.  There are 3 possible scenar-
ios: 
ℎ~
⎧
{
{
{
{
{
⎨
{
{
{
{
{
⎩
𝑙⁄
⁄
HMIN
HMAX < 𝑙
HMIN ≤ 𝑙 ≤ HMAX
0 < 𝑙 < HMIN
The ALE fluid must be modelled using the ALE single material with void ele-
ment  formulation  (ELFORM =  12)  because  the  LS-DYNA  thermal  solver  sup-
ports only one temperature per node.  However, a workaround enables partial 
support  for  ELFORM =11.    Rather  than  using  the  thermal  solver’s  nodal  tem-
perature  field,  the  ALE  temperature  is  derived  from  element’s  internal  energy 
using the heat capacity.  The heat is then extracted from or added to the internal 
energy  of  ALE  elements.    This  feature  was  implemented  to  calculate  the  heat 
exchange  between  a  gas  mixture,  modeled  with  *MAT_GAS_MIXTURE  and 
ALE multi-material formulation ELFORM = 11, and a Lagrangian container. 
HMIN < 0  turns  on  constraint-based  thermal  nodal  coupling  between  the  La-
grangian surface nodes and ALE fluid nodes.  This option only works with ALE 
single material with void element formulation (ELFORM = 12).  Once a Lagran-
gian  surface  node  is  in  contact  with  ALE  fluid  (gap =  0),  the  heat  transfer  de-
scribed above is turned off.  Instead the Lagrangian surface node temperature is 
constrained to the ALE fluid temperature field. 
9.  Leakage  Control.    The  dominate  force  preventing  leakage  across  a  coupled 
Lagrangian surface should be the penalty associated with the coupling.  Forces 
from the leakage control algorithm feature should be secondary.  The *DATA-
BASE_FSI  keyword  controls  the  “dbfsi”  file,  which  reports  both  the  coupling 
forces and the leakage control force contribution.  It is useful for debugging and 
fine-tuning.
ILEAK = 2 conserves energy; thus, it is better for airbag applications.  Leakage 
control  should  only  be  enabled  when  (1)  coupling  to  a  specific  AMMG 
(MCOUP as a negative integer) is activated, and (2) the fluid interface is clearly 
defined and tracked through the *ALE_MULTI-MATERIAL_GROUP card. 
10.  Pressure  Definition  in  Porous  Flow.    There  are  currently  two  methods  to 
model porous flow across a Lagrangian shell structure.  Both methods involve 
defining an empirical data curve of relative porous gas velocity as a function of 
system  pressure.    However  the  pressure  definitions  are  slightly  different  de-
pending on the choice of parameter defined: 
a)  When porous flow is modelled using the LCIDPOR parameter (part of this 
keyword), the velocity response curve expected to be given in terms of the 
pressure difference: 𝑃upstream − 𝑃downstream. 
b)  When  LCIDPOR  is  negative,  porous  flow  is  modelled  using  the  *MAT_-
FABRIC material model.  The FAC field in *MAT_FABRIC contains a load 
curve  ID  given  in  terms  of  absolute  upstream  pressure,  rather  than  in 
terms of the pressure difference. 
The  *AIRBAG_ALE  keyword  assumes  that  the  curve  referenced  by  FAC  in 
*MAT_FABRIC is given in terms of absolute upstream pressure.  These absolute 
pressure data are required for the CV phase.  During the ALE phase, LS-DYNA 
automatically shifts the FAC curve left (negative) by 1 atmospheric pressure for 
the  porous  coupling  calculation,  which  uses  gauge  pressure,  rather  than  abso-
lute pressure. 
The  mass  flowing  across  a  porous  Lagrangian  surface  can  be  tracked  by  the 
“pleak”  parameter  of  the  optional  “dbfsi”  ASCII  output  file,  which  may  be 
enabled with the *DATABASE_FSI keyword. 
11.  Venting.    There  are  2  methods  to  model  (airbag)  venting.    The  accumulated 
mass  output  of  both  may  be  tracked  via  the  *DATABASE_FSI  card  (“pleak” 
parameter in the “dbfsi” ASCII output file). 
a)  Isentropic Venting.  In isentropic venting, (define NVENT on card 3) the 
flow crossing the vent hole surface is estimated from the isentropic equa-
tion.  All airbag shell normal vectors should point uniformly in the same 
direction: typically, inward.  The shell elements for the vent holes, includ-
ed in the Lagrangian coupling set, should also point in the same direction 
as  the  airbag  meaning  usually  inward.    For  more  details  on  isentropic 
venting  see  *AIRBAG_WANG_NEFSKE  mass  flow  rate  equation  for  op-
tion OPT EQ.1 and 2. 
b)  Physical Venting.   Physical venting models  involve holes in the Lagran-
gian  structure  (usually  airbags).    The  shell  parts  representing  the  vent
holes may be either excluded from the Lagrangian coupling set, or, if in-
cluded, have normal vectors reversed from the rest of the airbag.  Typical-
ly,  this  means  the  holes  having  outward  facing  normal  vectors,  since  the 
rest  of  the  airbag  has  inward  pointing  normal  vectors.    With  either  ap-
proach the holes produce no coupling force to stop fluid leakage. 
When a particular AMMG is present on both sides of the same Lagrangi-
an  shell  surface,  penalty  coupling  can  break down.    Therefore, It  is  rec-
ommended  that  *ALE_FSI_SWITCH_MMG_ID  be  used  to  switch  the 
AMMG ID of the vented gas so that the vented gas outside the bag does 
not lead to leakage. 
12.  Initial  Penetration  Check.    Typically,  penetration  check  (IPENCHK)  should 
only be used if there is high coupling force applied at t=0.  For example, consid-
er  a  Lagrangian  container,  filled  with  non-gaseous  fluid  (i.e.    ALE  liquid  or 
solid) via the *INITIAL_VOLUME_FRACTON_GEOMETRY command.  Some-
times  due  to  mesh  resolution  or  complex  container  geometry,  there  is  initial 
penetration  of  the  fluid  across  the  container  surface.    This  can  give  rise  to  a 
sharp and immediate coupling force on the fluid at t=0.  Turning on IPENCHK 
may help eliminate this spike in coupling force. 
13.  Porous  Flow  for  Shell  Elements.    For  shell,  CTYPE=11,  the  Ergun-type 
empirical  porous  flow  equation  is  applied  to  the  normal  flow  direction  across 
the porous surface.  The pressure gradient along the segment normal direction 
is  
𝑑𝑃
𝑑𝑥𝑛
= 𝐴𝑛(𝜀, 𝜇)𝑉𝑛 + 𝐵𝑛(𝜀, 𝜌)|𝑉𝑛|𝑉𝑛 
where the subscript “n” refers to the direction normal to the porous Lagrangian 
shell surface and where, 
a)  𝑉𝑛  is  the  relative  normal-to-porous-shell-surface  fluid  velocity  compo-
nent. 
b)  𝐴𝑛(𝜀, 𝜇) = 𝐴1(𝜀, 𝜇)  is  a  viscous  coefficient  of  the  Ergun-type  porous  flow 
equation.    As  applied  here  it  should  contain  the  fluid  dynamic  viscosity, 
 𝜇 , and shell porosity,  𝜀  information. 
c)  𝐵𝑛(𝜀, 𝜌) = 𝐵1(𝜀, 𝜌) is an inertial coefficient of the Ergun-type porous flow 
equation.  As applied here it should contain the fluid density, 𝜌, and shell 
porosity, 𝜀, information. 
The force increment applied per segment is 
𝐹𝑛 =  
𝑑𝜌
𝑑𝑥𝑛
× THKF × 𝑆,
N5
N1
N8
Ez
N4
Ey
Ex
N6
N2
N7
N3
Figure  10-33.    The  Ex  direction  is  aligned  along  the  line  segment  connecting
the centers of  the 2-3-6-7 and the 1-4-8-5 faces.  The Ey direction is orthogonal
to  the  Ex  direction  and  in  the  plane  containing  both  Ex  and  containing  the
segment  connecting  the  centers  of  the  1-2-6-5  and  3-4-8-7  faces.    The  Ez  is
normal to this plane. 
where, 𝑆 is the segment surface area. 
If *DEFINE_POROUS_LAGRANGIAN defines the porous properties of a slave 
element,  the  porous  forces  are  computed  with  an  equation  similar  to  the  one 
used in *LOAD_BODY_POROUS  
NOTE:  𝐴𝑖(𝜀, 𝜇),  𝐵𝑖(𝜀, 𝜌),  and  THKF  are  required  input  for  porous 
shell coupling. 
14.  Porous  Flow  for  Solid  Elements.    For  porous  solid,  CTYPE=12,  the  pressure 
gradient along each global direction (i) can be computed similarly. 
𝑑𝑃
𝑑𝑥𝑖
= 𝐴𝑖(𝜀, 𝜇)𝑉𝑖 + 𝐵𝑖(𝜀, 𝜌)|𝑉𝑖|𝑉𝑖 for 𝑖 = 1,2,3 
Where, 
a)  𝑉𝑖 is the relative fluid velocity component through the porous solid in the 
3 global directions.  
b)  𝐴𝑖(𝜀, 𝜇) is a viscous coefficient of the Ergun-type porous flow equation in 
the ith direction.  As applied here it should contain the fluid dynamic vis-
cosity, 𝜇, and shell porosity, 𝜀, information.
c)  𝐵𝑖(𝜀, 𝜌) is an inertial coefficient of the Ergun-type porous flow equation in 
the  ith  direction.    As  applied  here  it  should  contain  the  fluid  density  (𝜌) 
and solid porosity (𝜀) information. 
NOTE:  𝐴𝑖(𝜀, 𝜇),  and  𝐵𝑖(𝜀, 𝜌)  are  required  input  for  porous  solid 
coupling. 
system 
If  DIREC = 1,  the  pressure  gradient  in  a  solid  is  applied  in  a  local  reference 
coordinate 
If 
*DEFINE_POROUS_LAGRANGIAN  defines  the  porous  properties  of  a  slave 
element,  the  local  system  can  be  adapted  and  the  porous  forces  are  computed 
with an equation similar to the one used in *LOAD_BODY_POROUS.
defined 
Figure 
10-33. 
in
*CONSTRAINED_LINEAR_GLOBAL 
Purpose:    Define  linear  constraint  equations  between  displacements  and  rotations, 
which can be defined in global coordinate systems. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
Type 
I 
Default 
none 
DOF  Card.    Define  one  card  for  each  constrained  degree-of-freedom.    Input  is 
terminated when a "*" card is found.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID 
DOF 
COEF 
Type 
I 
Default 
none 
Remark 
1 
  VARIABLE   
LCID 
I 
0 
I 
0 
DESCRIPTION
Linear constraint definition ID.  This ID can be used to identify a
set to which this constraint is a member. 
NID 
Node ID
VARIABLE   
DESCRIPTION
DOF 
Degree of freedom in the global coordinate system; 
EQ.1: displacement along global 𝑥-direction 
EQ.2: displacement along global 𝑦-direction 
EQ.3: displacement along global 𝑧-direction 
EQ.4: global rotation about global 𝑥-axis 
EQ.5: global rotation about global 𝑦-axis 
EQ.6: global rotation about global 𝑧-axis 
COEF 
Nonzero coefficient, 𝐶𝑘 
Remarks: 
Nodes of a nodal constraint equation cannot be members of another constraint equation 
or constraint set that constrain the same degrees-of-freedom, a tied interface, or a rigid 
body; i.e.  nodes cannot be subjected to multiple, independent, and possibly conflicting 
constraints.  Also care must be taken to ensure that single point constraints applied to 
nodes  in  a  constraint  equation  do  not  conflict  with  the  constraint  sets  constrained 
degrees-of-freedom. 
In this section linear constraint equations of the form: 
∑ 𝐶𝑘𝑢𝑘 = 𝐶0
𝑘=1
can  be  defined,  where  uk  are  the  displacements  and  Ck  are  user  defined  coefficients.  
Unless LS-DYNA is initialized by linking to an implicit code to satisfy this equation at 
the  beginning  of  the  calculation,  the  constant  C0  is  assumed  to  be  zero.    The  first 
constrained degree-of-freedom is eliminated from the equations-of-motion: 
its velocities and accelerations are given by 
𝑢1 = 𝐶0 − ∑
𝑘=2
𝐶𝑘
𝐶1
𝑢𝑘 
𝑢̇1 = − ∑
𝑘=2
𝑢̈1 = − ∑
𝑘=2
𝐶𝑘
𝐶1
𝐶𝑘
𝐶1
𝑢̇𝑘 
𝑢̈𝑘, 
respectively.  In the implementation a transformation matrix, 𝐋, is constructed relating 
the  unconstrained,  𝐮,  and  constrained,  𝐮𝑐,  degrees-of-freedom.    The  constrained 
accelerations used in the above equation are given by:
𝐮̈𝑐 = [𝐋T𝐌𝐋]−1𝐋T𝐅 
where 𝐌 is the Diagonal lumped mass matrix and 𝐅 is the right hand side force vector.  
This requires the inversion of the condensed mass matrix which is equal in size to the 
number of constrained degrees-of-freedom minus one. 
Example: 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *CONSTRAINED_LINEAR_GLOBAL 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Constrain nodes 40 and 42 to move identically in the z-direction. 
$ 
$  When the linear constraint equation is applied, it goes like this: 
$ 
$     0 = C40uz40 + C42uz42 
$ 
$       = uz40 - uz42 
$ 
$     uz40 = uz42 
$ 
$   where, 
$     C40  =  1.00  coefficient for node 40 
$     C42  = -1.00  coefficient for node 42 
$     uz40 = displacement of node 40 in z-direction 
$     uz42 = displacement of node 42 in z-direction 
$ 
$ 
*CONSTRAINED_LINEAR 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$        i 
$       id 
         2 
$ 
$      nid       dof     coef 
        40         3     1.00 
        42         3    -1.00 
$ 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$
*CONSTRAINED_LINEAR_LOCAL 
Purpose:    Define  linear  constraint  equations  between  displacements  and  rotations, 
which  can  be  defined  in  a  local  coordinate  system.    Each  node  may  have  a  unique 
coordinate ID.   
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
Type 
I 
Default 
none 
DOF  Cards.    Define  one  card  for  each  constrained  degree-of-freedom.    Input  is 
terminated at next “*” card.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID 
DOF 
CID 
COEF 
Type 
I 
Default 
none 
Remark 
1 
  VARIABLE   
LCID 
I 
0 
I 
0 
I 
0 
DESCRIPTION
LCID  for  linear  constraint  definition.    This  ID  can  be  used  to
identify a set to which this constraint is a member. 
NID 
Node ID
VARIABLE   
DESCRIPTION
DOF 
Degree of freedom in the local coordinate system; 
EQ.1: displacement along local x-direction 
EQ.2: displacement along local y-direction 
EQ.3: displacement along local z-direction 
EQ.4: local rotation about local x-axis 
EQ.5: local rotation about local y-axis 
EQ.6: local rotation about local z-axis 
CID 
Local  coordinate  system  ID  number.    If  the  number  is  zero,  the
global coordinate system is used. 
COEF 
Nonzero coefficient, Ck 
Remarks: 
In this section linear constraint equations of the form: 
∑ 𝐶𝑘
𝑘=1
𝐿 = 𝐶0 
𝑢𝑘
𝐿 are the displacements in the local coordinate systems and Ck 
can be defined, where 𝑢𝑘
are  user  defined  coefficients.    Unless  LS-DYNA  is  initialized  by  linking  to  an  implicit 
code  to  satisfy  this  equation  at  the  beginning  of  the  calculation,  the  constant  C0  is 
assumed  to  be  zero.    The  first  constrained  degree-of-freedom  is  eliminated  from  the 
equations-of-motion: 
Its velocities and accelerations are given by 
𝐿 = 𝐶0 − ∑
𝑢1
𝑘=2
𝐶𝑘
𝐶1
𝐿 
𝑢𝑘
𝐿 = − ∑
𝑢̇1
𝑘=2
𝐿 = − ∑
𝑢̈1
𝑘=2
𝐶𝑘
𝐶1
𝐶𝑘
𝐶1
𝑢̇𝑘
𝑢̈𝑘
respectively.    The  local  displacements  are  calculated  every  time  step  using  the  local 
coordinate systems defined by the user.   More than one degree of freedom for a node 
can be constrained by specifying a card for each degree of freedom.
WARNING:  Nodes of a nodal constraint equation cannot be mem-
bers  of  another  constraint  equation  or  constraint  set 
that contains the same degrees-of-freedom, tied inter-
face, or rigid bodies. 
Nodes  must  not  be  subject  to  multiple,  independent, 
and  possibly  conflicting  constraints.    Furthermore, 
care  must  be  taken  to  ensure  that  single  point  con-
straints  applied  to  nodes  in  a  constraint  equation  do 
not  conflict  with  the  constraint  set’s  constrained  de-
grees-of-freedom.
Purpose:  Define a local boundary constraint plane. 
*CONSTRAINED 
  Card 1 
Variable 
Type 
Default 
1 
TC 
1 
0 
2 
RC 
1 
0 
3 
DIR 
1 
0 
4 
X 
F 
0 
5 
Y 
F 
0 
8 
6 
Z 
F 
0 
7 
CID 
1 
none 
  VARIABLE   
DESCRIPTION
TC 
Translational Constraint in local system: 
EQ.1: constrained x translation, 
EQ.2: constrained y translation, 
EQ.3: constrained z translation, 
EQ.4: constrained x and y translations, 
EQ.5: constrained y and z translations, 
EQ.6: constrained x and z translations, 
EQ.7: constrained x, y, and translations. 
RC 
Rotational Constraint in local system: 
EQ.1: constrained x-rotation, 
EQ.2: constrained y-rotation, 
EQ.3: constrained z-rotation, 
EQ.4: constrained x and y rotations, 
EQ.5: constrained y and z rotations, 
EQ.6: constrained z and x rotations, 
EQ.7: constrained x, y, and z rotations.
VARIABLE   
DESCRIPTION
DIR 
Direction of normal for local constraint plane. 
EQ.1: local x, 
EQ.2: local y, 
EQ.3: local z. 
Local x-coordinate of a point on the local constraint plane. 
Local y-coordinate of a point on the local constraint plane. 
Local z-coordinate of a point on the local constraint plane. 
Coordinate  system  ID  for  orientation  of  the  local  coordinate
system. 
X 
Y 
Z 
CID 
Remarks: 
Nodes  within  a  mesh-size-dependent  tolerance  are  constrained  on  a  local  plane.    This 
option  is  recommended  for  use  with  r-method  adaptive  remeshing  where  nodal 
constraints are lost during the remeshing phase.
*CONSTRAINED_MULTIPLE_GLOBAL 
Purpose:    Define  global  multi-point  constraints  for  imposing  periodic  boundary 
condition in displacement field. 
2 
3 
4 
5 
6 
7 
8 
  Card 1 
Variable 
1 
ID 
Type 
I 
Default 
NOTE:  For  each  constraint  equation  include  a  set  of  cards  consisting  of 
(1)  a  Constraint  Equation  Definition  Card  and  (2)  NMP  Coefficient 
Cards. 
Constraint Equation Definition Card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NMP 
Type 
I 
Default 
Coefficient Cards.  The next NMP cards adhere to this format.  Each card sets a single 
coefficient in the constraint equation. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID 
DIR 
COEF 
Type 
I 
I 
F 
Default
11 
8 
5 
7 
4 
*CONSTRAINED_MULTIPLE_GLOBAL 
9 
6 
1 
3 
 3, 1, 1.0 
 1, 1,-1.0 
10 
10, 1,-1.0 
(3) − 𝑢1
𝑢1
(1) − 𝑢1
(10) = 0 
1 
2 
3 
3 
 8, 1, 1.0 
 2, 1,-1.0 
11, 1,-1.0 
(8) − 𝑢1
𝑢1
(2) − 𝑢1
(11) = 0 
*CONSTRAINED_MULTIPLE_GLOBAL 
2 
3 
 3, 2, 1.0 
 1, 2,-1.0 
10, 2,-1.0 
(3) − 𝑢2
𝑢2
(1) − 𝑢2
(10) = 0 
Figure 10-34.  Simple example. 
  VARIABLE   
DESCRIPTION
ID 
Constraint  set  identification.    All  constraint  sets  should  have  a
unique set ID. 
NMP 
Number of nodes to be constrained mutually. 
NID 
DIR 
Nodal ID 
Direction in three-dimensional space to be constrained 
EQ.1: 𝑥 direction 
EQ.2: 𝑦 direction 
EQ.3: 𝑧 direction 
LT.0:  Extra DOFs for user defined element formulation (e.g.  -
1: the 1st extra DOF; -2: the 2nd extra DOF; …)
VARIABLE   
DESCRIPTION
COEF 
Coefficient 𝛼NID in constraint equation: 
∑ 𝛼NID𝑢DIR
NID
(NID) = 0
.
Remarks: 
1.  Defining  multi-point  constraints  by  this  keyword  can  be  demonstrated  by  the 
following  example:  a two-dimensional  unit  square  with  four  quadrilateral  ele-
ments and 11 nodes as shown in the figure below, where the nodes #10 and #11 
are two dummy nodes serving as control points.
*CONSTRAINED_NODAL_RIGID_BODY_{OPTION}_{OPTION}_{OPTION} 
Available options include: 
<BLANK> 
SPC 
INERTIA 
TITLE 
If  the  center  of  mass  is  constrained  use  the  SPC  option.    If  the  inertial  properties  are 
defined  rather  than  computed  use  the  INERTIA  option.    A  description  for  the  nodal 
rigid body can be defined with the TITLE option. 
Purpose:  Define a nodal rigid body.  This is a rigid body which consists of the defined 
nodes.  If the INERTIA option is not used, then the inertia tensor is computed from the 
nodal masses.  Arbitrary motion of this rigid body is allowed.  If the INERTIA option is 
used, constant translational and rotational velocities can be defined in a global or local 
coordinate system.   
The  first  node  in  the  nodal  rigid  body  definition  is  treated  as  the  master  for  the  case 
where  DRFLAG  and  RRFLAG  are  nonzero.    The  first  node  always  has  six  degrees-of-
freedom.  The release conditions applied in the global system are sometimes convenient 
in  small  displacement  linear  analysis,  but,  otherwise,  are  not  recommended.    It  is 
strongly  recommended,  especially  for  implicit  calculations,  that  release  conditions  are 
only used for a two noded nodal rigid body. 
Card Format: 
Card 1: 
required 
Card 2: 
required for SPC option 
Card 3 - 5: 
required for INERTIA option 
Card 6: 
required if a local coordinate system is used to specify the inertia 
tensor when the INERTIA option is set 
Remarks: 
1.  Unlike  the  *CONSTRAINED_NODE_SET  which  permits  only  constraints  on 
translational  motion,  here  the  equations  of  rigid  body  dynamics  are  used  to 
update  the  motion  of  the  nodes  and  therefore  rotations  of  the  nodal  sets  are 
admissible.    Mass  properties  are  determined  from  the  nodal  masses  and  coor-
dinates.    Inertial  properties  are  defined  if  and  only  if  the  INERTIA  option  is 
specified. 
Title Card.  Additional card for the TITLE keyword option.  
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
TITLE 
A80 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
CID 
NSID 
PNODE 
IPRT 
DRFLAG 
RRFLAG 
Type 
I 
I 
I 
Default 
none 
none 
none 
I 
0 
I 
0 
I 
0 
I 
0 
Center of Mass Constraint Card.  Additional card for the SPC keyword option. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CMO 
CON1 
CON2 
Type 
Default 
F 
0 
F 
0 
F 
0 
  VARIABLE   
DESCRIPTION
PID 
CID 
Part ID of the nodal rigid body. 
Optional coordinate system ID for the rigid body local system, see
*DEFINE_COORDINATE_OPTION.    Output  of  the  rigid  body 
data  and  the  degree-of-  freedom  releases  are  done  in  this  local 
system.  This local system rotates with the rigid body.
VARIABLE   
NSID 
PNODE 
DESCRIPTION
Nodal  set  ID,  see  *SET_NODE_OPTION.    This  nodal  set  defines 
the rigid body.  If NSID = 0, then NSID = PID, i.e., the node set ID 
and the part ID are assumed to be identical. 
An  optional  node  (a  massless  node  is  allowed)  used  for  post
processing  rigid  body  data.    If  the  PNODE  is  not  located  at  the
rigid body’s center of mass, then the initial coordinates of PNODE
will be reset to the center of mass.  If CID is defined, the velocities
and accelerations of PNODE will be output in the local system to
the  d3plot  and  d3thdt  files  unless  PNODE  is  specified  as  a 
negative number, in which case the global system is used. 
IPRT 
Print flag.  For nodal rigid bodies the following values apply: 
EQ.1:  write data into rbdout 
EQ.2:  do not write data into rbdout 
Printing is suppressed for two noded rigid bodies unless IPRT is
set to unity.  This is to avoid excessively large rbdout files  when 
many, two-noded welds are used. 
DRFLAG 
Displacement release flag for all nodes except the first node in the
definition. 
EQ.-7:  release 𝑥, 𝑦, and 𝑧 displacement in global system 
EQ.-6:  release 𝑧 and 𝑥 displacement in global system 
EQ.-5:  release 𝑦 and 𝑧 displacement in global system 
EQ.-4:  release 𝑥 and 𝑦 displacement in global system 
EQ.-3:  release 𝑧 displacement in global system 
EQ.-2:  release 𝑦 displacement in global system 
EQ.-1:  release 𝑥 displacement in global system 
EQ.0:  off for rigid body behavior 
EQ.1:  release 𝑥 displacement in rigid body local system 
EQ.2:  release 𝑦 displacement in rigid body local system 
EQ.3:  release 𝑧 displacement in rigid body local system 
EQ.4:  release 𝑥 and 𝑦 displacement in rigid body local system
EQ.5:  release 𝑦 and 𝑧 displacement in rigid body local system 
EQ.6:  release 𝑧 and 𝑥 displacement in rigid body local system 
EQ.7:  release  𝑥,  𝑦,  and  𝑧  displacement  in  rigid  body  local
VARIABLE   
DESCRIPTION
system 
RRFLAG 
Rotation  release  flag  for  all  nodes  except  the  first  node  in  the
definition. 
EQ.-7:  release 𝑥, 𝑦, and 𝑧 rotations in global system 
EQ.-6:  release 𝑧 and 𝑥 rotations in global system 
EQ.-5:  release 𝑦 and 𝑧 rotations in global system 
EQ.-4:  release 𝑥 and 𝑦 rotations in global system 
EQ.-3:  release 𝑧 rotation in global system 
EQ.-2:  release 𝑦 rotation in global system 
EQ.-1:  release 𝑥 rotation in global system 
EQ.0:  off for rigid body behavior 
EQ.1:  release 𝑥 rotation in rigid body local system 
EQ.2:  release 𝑦 rotation in rigid body local system 
EQ.3:  release 𝑧 rotation in rigid body local system 
EQ.4:  release 𝑥 and 𝑦 rotations in rigid body local system 
EQ.5:  release 𝑦 and 𝑧 rotations in rigid body local system 
EQ.6:  release 𝑧 and 𝑥 rotations in rigid body local system 
EQ.7:  release 𝑥, 𝑦, and 𝑧 rotations in rigid body local system 
CMO 
Center of mass constraint option, CMO: 
EQ.+1.0:  constraints applied in global directions, 
EQ.0.0:  no constraints, 
EQ.-1.0:  constraints  applied 
constraint). 
in 
local  directions 
(SPC
CON1 
First constraint parameter: 
If CMO=+1.0, then specify global translational constraint: 
EQ.0:  no constraints, 
EQ.1:  constrained 𝑥 displacement, 
EQ.2:  constrained 𝑦 displacement, 
EQ.3:  constrained 𝑧 displacement, 
EQ.4:  constrained 𝑥 and 𝑦 displacements,
VARIABLE   
DESCRIPTION
EQ.5:  constrained 𝑦 and 𝑧 displacements, 
EQ.6:  constrained 𝑧 and 𝑥 displacements, 
EQ.7:  constrained 𝑥, 𝑦, and 𝑧 displacements. 
If  CM0 = -1.0,  then  specify  local  coordinate  system  ID.    See  *DE-
FINE_COORDINATE_OPTION:    This  coordinate  system  is  fixed 
in time 
CON2 
Second constraint parameter: 
If CMO=+1.0, then specify global rotational constraint: 
EQ.0:  no constraints, 
EQ.1:  constrained 𝑥 rotation, 
EQ.2:  constrained 𝑦 rotation, 
EQ.3:  constrained 𝑧 rotation, 
EQ.4:  constrained 𝑥 and 𝑦 rotations, 
EQ.5:  constrained 𝑦 and 𝑧 rotations, 
EQ.6:  constrained 𝑧 and 𝑥 rotations, 
EQ.7:  constrained 𝑥, 𝑦, and 𝑧 rotations. 
If CM0 = -1.0, then specify local (SPC) constraint: 
EQ.000000:  no constraint, 
EQ.100000:  constrained 𝑥 translation, 
EQ.010000:  constrained 𝑦 translation, 
EQ.001000:  constrained 𝑧 translation, 
EQ.000100:  constrained 𝑥 rotation, 
EQ.000010 :  constrained 𝑦 rotation, 
EQ.000001:  constrained 𝑧 rotation. 
Any  combination  of  local  constraints  can  be  achieved  by  adding
the number 1 into the corresponding column.
Inertia Card 1.  Additional card for the INERTIA keyword option.  
  Card 3 
Variable 
Type 
Default 
1 
XC 
F 
0 
2 
YC 
F 
0 
3 
ZC 
F 
0 
4 
TM 
F 
0 
5 
6 
7 
8 
IRCS 
NODEID 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
XC 
YC 
ZC 
TM 
𝑥-coordinate  of  center  of  mass.    If  nodal  point,  NODEID,  is
defined,  XC,  YC,  and  ZC  are  ignored  and  the  coordinates  of  the
nodal point, NODEID, are taken as the center of mass. 
𝑦-coordinate of center of mass 
𝑧-coordinate of center of mass 
Translational mass 
IRCS 
Flag for inertia tensor reference coordinate system: 
EQ.0:  global inertia tensor, 
EQ.1:  local  inertia  tensor  is  given  in  a  system  defined  by  the
orientation vectors as given below. 
NODEID 
Optional  nodal  point  defining  the  CG  of  the  rigid  body.    If  this
node is not a member of the set NSID above, its motion will  not
be  updated  to  correspond  with  the  nodal  rigid  body  after  the
calculation begins.  PNODE and NODEID can be identical if and
only if PNODE physically lies at the mass center at time zero.
Inertia Card 2.  Second Additional card for the INERTIA keyword option. 
  Card 4 
1 
Variable 
IXX 
Type 
F 
Default 
none 
2 
IXY 
F 
0 
3 
IXZ 
F 
0 
4 
IYY 
F 
none 
5 
IYZ 
F 
0 
6 
IZZ 
F 
0 
7 
8 
  VARIABLE   
DESCRIPTION
IXX 
IXY 
IXZ 
IYY 
IYZ 
IZZ 
𝐼𝑥𝑥, 𝑥𝑥 component of inertia tensor 
𝐼𝑥𝑦, 𝑥𝑦 component of inertia tensor 
𝐼𝑥𝑧, 𝑥𝑧 component of inertia tensor 
𝐼𝑦𝑦, 𝑦𝑦 component of inertia tensor 
𝐼𝑦𝑧, 𝑦𝑧 component of inertia tensor 
𝐼𝑧𝑧, 𝑧𝑧 component of inertia tensor 
Inertia Card 3.  Third additional card for the INERTIA keyword option.  
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VTX 
VTY 
VTZ 
VRX 
VRY 
VRZ 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
  VARIABLE   
DESCRIPTION
VTX 
VTY 
𝑥-rigid  body  initial  translational  velocity  in  global  coordinate
system. 
𝑦-rigid  body  initial  translational  velocity  in  global  coordinate
system.
VARIABLE   
DESCRIPTION
VTZ 
VRX 
VRY 
𝑧-rigid  body  initial  translational  velocity  in  global  coordinate
system. 
𝑥-rigid  body  initial  rotational  velocity  in  global  coordinate 
system. 
𝑦-rigid  body  initial  rotational  velocity  in  global  coordinate
system. 
VRZ 
𝑧-rigid body initial rotational velocity in global coordinate system.
Remarks: 
The velocities defined above can be overwritten by the *INITIAL_VELOCITY card. 
Local Inertia Tensor Card.  Additional card required for IRCS = 1 . 
Define two local vectors or a local coordinate system ID.  
  Card 6 
Variable 
1 
XL 
Type 
F 
2 
YL 
F 
3 
ZL 
F 
4 
5 
6 
7 
8 
XLIP 
YLIP 
ZLIP 
CID2 
F 
F 
F 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
XL 
YL 
ZL 
XLIP 
YLIP 
ZLIP 
CID2 
𝑥-coordinate of local 𝑥-axis.  Origin lies at (0,0,0). 
𝑦-coordinate of local 𝑥-axis 
𝑧-coordinate of local 𝑥-axis 
𝑥-coordinate of local in-plane vector 
𝑦-coordinate of local in-plane vector 
𝑧-coordinate of local in-plane vector 
Local  coordinate  system  ID,  see  *DEFINE_COORDINATE_.... 
With this option leave fields 1-6 blank.
Remarks: 
The  local  coordinate  system  is  set  up  in  the  following  way.    After  the  local  x-axis  is 
defined,  the  local  𝑧-axis  is  computed  from  the  cross-product  of  the  local  𝑥-axis  vector 
with  the  given  in-plane  vector.    Finally,  the  local  𝑦-axis  is  determined  from  the  cross-
product of the local 𝑧-axis with the local 𝑥-axis.  The local coordinate system defined by 
CID has the advantage that the local system can be defined by nodes in the rigid body 
which  makes  repositioning  of  the  rigid  body  in  a  preprocessor  much  easier  since  the 
local system moves with the nodal points. 
Example: 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *CONSTRAINED_NODAL_RIGID_BODY 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Define a rigid body consisting of the nodes in nodal set 61. 
$ 
$  This particular example was used to connect three separate deformable  
$  parts.  Physically, these parts were welded together.  Modeling wise, 
$  however, this joint is quit messy and is most conveniently modeled 
$  by making a rigid body using several of the nodes in the area.  Physically, 
$  this joint was so strong that weld failure was never of concern. 
$ 
*CONSTRAINED_NODAL_RIGID_BODY 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      pid       cid      nsid 
        45                  61 
$ 
$     nsid = 61   nodal set ID number, requires a *SET_NODE_option 
$      cid        not used in this example, output will be in global coordinates 
$ 
$ 
*SET_NODE_LIST 
$      sid 
        61 
$     nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
       823      1057      1174      1931      2124      1961      2101 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
*CONSTRAINED_NODE_INTERPOLATION 
Purpose:    Define  constrained  nodes  for  the  use  of  *ELEMENT_INTERPOLATION_-
SHELL  and  *ELEMENT_INTERPOLATION_SOLID  to  model  contact  and  to  visualize 
the  results  of generalized  elements  .  
The displacements of these nodes are dependent of their corresponding master nodes. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID 
NUMMN 
Type 
I 
I 
Default 
none 
none 
Weighting  Factor  Cards.    For  each  of  the  NUMMN  master  nodes    NID  depends  on  set  a  MN  and  W  entry.    Each 
Weighting Factor Card can accommodate four master nodes.  Add as many Weighting 
Factor Cards as needed. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MN1 
W1 
MN2 
W2 
MN3 
W3 
MN4 
W4 
Type 
I 
F 
I 
F 
I 
F 
I 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 3 
1 
Variable 
MN5 
2 
W5 
3 
4 
5 
6 
7 
8 
Etc. 
Etc. 
Etc. 
Etc. 
Etc. 
Etc. 
Type 
I 
F 
I 
F 
I 
F 
I 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none
26
25
24
15
14
16
26
25
78
16
15
Connectivity of
Generalized-Shell Element
Generalized-Shell Element
(*ELEMENT_GENERALIZED_SHELL)
Interpolation Node
(*CONSTRAINED_NODE_INTERPOLATION)
Interpolation Element
(*ELEMENT_INTERPOLATION_SHELL)
*CONSTRAINED_NODE_INTERPOLATION
$---+--NID----+NUMCN----+----3----+----4----+----5----+----6----+----7----+----8
78
$---+--CN1----+---W1----+--CN2----+---W2----+--CN3----+---W3----+--CN4----+---W4
0.15
0.32 
0.18 
0.35 
26 
25 
16 
15 
Figure  10-35.    Example  of  a  *CONSTRAINED_NODE_INTERPOLATION
card 
  VARIABLE   
NID 
DESCRIPTION
Node  ID  of  the  interpolation  node  as  defined  in  *NODE  . 
NUMMN 
Number of master nodes, this constrained node depends on. 
Node ID of master node i. 
Weighting factor of master node i. 
MNi 
Wi 
Remarks: 
1.  The coordinates of an interpolation node have to be defined in *NODE.  In there 
the translational and rotational constraints TC = 7.  and RC = 7.  need to be set. 
2.  The displacements of the interpolation node, 𝒅IN, are interpolated based on the 
displacements  of  the  corresponding  master  nodes,  𝒅𝑖,  and  the  appropriate 
weighting factors 𝑤𝑖.  The interpolation is computed as follows: 
NUMMN
𝒅IN = ∑ 𝑤𝑖𝒅𝑖
𝑖=1
.
*CONSTRAINED_NODE_SET_{OPTION} 
To define an ID for the constrained node set the following option is available: 
<BLANK> 
ID 
If the ID is defined an additional card is required. 
Purpose:    Define  nodal  constraint  sets  for  translational  motion  in  global  coordinates.  
No rotational coupling.  See Figure 10-36.  Nodal points included in the sets should not 
be  subjected  to  any  other  constraints  including  prescribed  motion,  e.g.,  with  the 
*BOUNDARY_PRESCRIBED_MOTION options. 
ID Card.  Additional card for ID keyword option. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CNSID 
Type 
Default 
I 
0 
  Card 2 
1 
2 
Variable 
NSID 
DOF 
Type 
I 
I 
3 
TF 
F 
Default 
none 
none 
1.E+20
Remarks 
1 
2 
4 
5 
6 
7 
8 
  VARIABLE   
DESCRIPTION
CNSID 
Optional constrained node set ID. 
NSID 
Nodal set ID, see *SET_NODE_OPTION.
Since no rotation is permitted, this 
option should not be used to model 
rigid  body  behavior 
involving 
rotations
*CONSTRAINED_NODE_SET 
*CONSTRAINED_NODAL_RIGID_BODY
*CONSTRAINED_SPOTWELD
Behavior  is  like  a  rigid  beam.    These 
options may be used to model spotwelds.
Figure  10-36.    Two  different  ways  to  constrain  node  𝑎  and 𝑏.    For rigid-body 
type  situations    this  card,  *CONSTRAINED_NODE_SET  may  lead  to  un-
physical results. 
  VARIABLE   
DESCRIPTION
DOF 
Applicable degrees-of-freedom: 
EQ.1: x-translational degree-of-freedom, 
EQ.2: y-translational degree-of-freedom, 
EQ.3: z-translational degree-of-freedom, 
EQ.4: x and y-translational degrees-of-freedom, 
EQ.5: y and z-translational degrees-of-freedom, 
EQ.6: z and x-translational degrees-of-freedom, 
EQ.7: x, y, and z-translational degrees-of-freedom. 
TF 
Failure time for nodal constraint set. 
Remarks: 
1.  The  masses  of  the  nodes  are  summed  up  to  determine  the  total  mass  of  the 
constrained set.  It must be noted that the definition of a nodal rigid body is not 
possible  with  this  input  For  nodal  rigid  bodies  the  keyword  input:  *CON-
STRAINED_NODAL_RIGID_BODY_OPTION, must be used. 
2.  When the failure time, TF, is reached the nodal constraint becomes inactive and 
the constrained nodes may move freely.
Example: 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *CONSTRAINED_NODE_SET 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Constrain all the nodes in a nodal set to move equivalently 
$  in the z-direction. 
$ 
*CONSTRAINED_NODE_SET 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
      nsid       dof        tf 
         7         3      10.0 
$ 
$     nsid = 7    nodal set ID number, requires a *SET_NODE_option 
$      dof = 3    nodal motions are equivalent in z-translation 
$      tf  = 3    at time=10.  the nodal constraint is removed 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$
*CONSTRAINED_NODE_TO_NURBS_PATCH_{OPTION} 
Purpose:    To  add  additional  massless  nodes  to  the  surface  of  a  NURBS  patch.    The 
motion of the nodes is governed by the NURBS patch.  Forces applied to the nodes are 
distributed  to  the  NURBS  patch.    Penalty  method  is  used  to  handle  the  displacement 
boundary conditions CON  on the specified nodes. 
To specify node sets instead of individual nodes use the option: 
SET 
6 
7 
8 
  Card 1 
1 
2 
3 
4 
Variable 
PATCHID 
NSID 
CON 
CID 
Type 
I 
I 
Default 
none 
none 
I 
I 
0 
5 
SF 
F 
1.0 
  VARIABLE   
DESCRIPTION
PATCHID 
Patch ID. 
NSID 
CON 
CID 
SF 
Nodal set ID or node ID depending on the OPTION. 
Constraint  parameter for  extra  node(s)  of  NSID.    Its  definition  is
in 
same  as  that  of  CON2  when  CM0 = -1  as  described 
MAT_RIGID. 
  For  example  “1110”  means  constrained  𝑧-
translation, 𝑥-rotation and 𝑦-rotation.   
Coordinate system ID for constraint 
Penalty force scale factor for the penalty-based constraint
*CONSTRAINED 
Purpose:    Constrain  two  points  with  the  specified  coordinates  connecting  two  shell 
elements  at  locations  other  than  nodal  points.    In  this  option,  the  penalty  method  is 
used  to  constrain  the  translational  and  rotational  degrees-of-freedom  of  the  points.  
Force resultants are written into the swforc ASCII file for post-processing. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CID 
Type 
I 
Default 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
EID1 
Type 
I 
Default 
none 
X1 
F 
0. 
Y1 
F 
0. 
Z1 
F 
0. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
EID2 
Type 
I 
Default 
none 
X2 
F 
0. 
Y2 
F 
0. 
Z2 
F 
0.
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PSF 
FAILA 
FAILS 
FAILM 
Type 
F 
F 
F 
F 
Default 
1.0 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
CID 
EIDi 
Constrained points ID. 
Shell element ID, i = 1, 2. 
Xi, Yi, Zi 
Coordinates of the constrained points, i = 1, 2. 
PSF 
Penalty scale factor (Default = 1.0). 
FAILA 
Axial force resultant failure value, no failure if zero. 
FAILS 
Shear force resultant failure value, no failure if zero. 
FAILM 
Moment resultant failure value, no failure if zero.
*CONSTRAINED_RIGID_BODIES 
Purpose:  Merge two rigid bodies.  One rigid body, called slave rigid body, is merged to 
the other one called a master rigid body.   This command applies to parts comprised of 
*MAT_RIGID 
bodies 
(*CONSTRAINED_NODAL_RIGID_BODY). 
nodal 
rigid 
but 
not 
to 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PIDM 
PIDS 
IFLAG 
Type 
I 
I 
Default 
none 
none 
I 
0 
  VARIABLE   
DESCRIPTION
PIDM 
PIDS 
IFLAG 
Master rigid body part ID, see *PART. 
Slave rigid body part ID, see *PART. 
This  flag  is  meaningful  if  and  only  if  the  inertia  properties  of  the 
Part, PIDM, are defined in PART_INERTIA.   
EQ.1:  Update the center-of-gravity, the translational mass, and 
the inertia matrix of PIDM to reflect its merging with the
slave rigid body (PIDS). 
EQ.0:  The merged PIDS will not affect the properties defined in 
PART_INERTIA for PIDM since it is assumed the prop-
erties  already  account  for  merged  parts.    The  inertia
properties  of  PIDS  will  be  computed  from  its  nodal
masses  if  the  properties  are  not  defined  in  a  PART_IN-
ERTIA definition. 
Remarks: 
1.  The slave rigid body is merged to the master rigid body.  The inertial properties 
computed by LS-DYNA are based on the combination of the master rigid body 
plus all the rigid bodies which are slaved to it unless the inertial properties of 
the master rigid body are defined via the *PART_INERTIA keyword in which 
case those properties are used for the combination of the master and slave rigid 
bodies.  Note that a master rigid body may have many slaves.
2. 
3. 
Independent rigid bodies must not share common nodes since each rigid body 
updates  the  motion  of  its  nodes  independently  of  the  other  rigid  bodies.    If 
common  nodes  exist  between  rigid  bodies  the  rigid  bodies  sharing  the  nodes 
must be merged. 
It is also possible to merge rigid bodies that are completely separated and share 
no common nodal points or boundaries.  All actions valid for the master rigid 
body, e.g., constraints, given velocity, are now also valid for the newly-created 
rigid body. 
Example: 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *CONSTRAINED_RIGID_BODIES 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Rigidly connect parts 35, 70, 71, and 72 to part 12. 
$  All parts must be defined as rigid. 
$ 
$  This example is used to make a single rigid body out of the five parts 
$  that compose the back end of a vehicle.  This was done to save cpu time 
$  and was determined to be valid because the application was a frontal 
$  impact with insignificant rear end deformations.  (The cpu time saved 
$  was from making the parts rigid, not from merging them - merging was 
$  more of a convenience in this case for post processing, for checking 
$  inertial properties, and for joining the parts.) 
$ 
*CONSTRAINED_RIGID_BODIES 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$     pidm      pids 
        12        35 
        12        70 
        12        71 
        12        72 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
*CONSTRAINED_RIGID_BODY_INSERT 
Purpose:  This keyword is for modeling die inserts.  One rigid body, called slave rigid 
body, is constrained to move with another rigid body, called the master rigid body, in 
all directions except for one. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
PIDM 
PIDS 
COORDID
IDIR 
Type 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
Variable  MFLAG 
MCID 
DEATHM 
I 
3 
5 
6 
7 
8 
F 
0.0 
3 
4 
5 
6 
7 
8 
Type 
Default 
I 
0 
  Card 3 
1 
I 
0 
2 
Variable 
PARTB 
DEATHB 
Type 
Default 
I 
0 
F 
0.0 
  VARIABLE   
DESCRIPTION
ID 
PIDM 
PIDS 
Insert ID 
Master (die) rigid body part ID, see *PART. 
Slave (die insert) rigid body part ID, see *PART.
VARIABLE   
COORDID 
DESCRIPTION
Coordinate  ID.    The  𝑥  direction  is  the  direction  the  insert  moves 
independently of the die. 
IDIR 
The  direction  the  insert  moves  independently  of  the  die.    If
unspecified, it defaults to the local z direction, IDIR = 3. 
MFLAG 
Motion flag.  
EQ.0: Relative motion is unconstrained. 
EQ.1:  The  displacement  of  the  insert  relative  to  the  die  is
imposed. 
EQ.2: The velocity of the insert relative to the die is imposed. 
EQ.3: The  acceleration  of  the  insert  relative  to  the  die  is
imposed. 
MCID 
Curve defining the motion of the die insert relative to the die. 
DEATHM 
Death time of the imposed motion.  If it is equal to 0.0, the motion
is imposed for the entire analysis. 
PARTB 
Part ID for a discrete beam connected between the insert and die.
DEATHB 
Death time for the discrete beam specified by BPART. 
Remarks: 
1.  This  capability  is  supported  by  both  the  implicit  and  explicit  time  integrators; 
however, the joint death time DEATHM feature works only for explicit integra-
tion with the penalty method. 
2.  The translational joint constraining the die and the die insert are automatically 
generated.  The joint reaction forces will appear in the jntforc output file. 
3.  The  translational  motor  constraining  the  remaining  translational  degree  of 
freedom  is  also  automatically  generated,  and  its  reaction  forces  also  appear  in 
the jntforc output file. 
4.  The automatically generated beam has its data written to the d3plot file, and all 
of the optional appropriate output files.
*CONSTRAINED_RIGID_BODY_STOPPERS 
Purpose:    Rigid  body  stoppers  provide  a  convenient  way  of  controlling  the  motion  of 
rigid  tooling  in  metalforming  applications.    The  motion  of  a  “master”  rigid  body  is 
limited  by  load  curves.    This  option  will  stop  the  motion  based  on  a  time  dependent 
constraint.    The  stopper  overrides  prescribed  motion  boundary  conditions  (except 
relative  displacement)  operating  in  the  same  direction  for  both  the  master  and  slaved 
rigid bodies.  See Figure 10-37. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
Variable 
PID 
LCMAX 
LCMIN 
PSIDMX 
PSIDMN 
LCVMNX 
DIR 
8 
VID 
I 
0 
3 
I 
0 
4 
I 
0 
5 
I 
I 
I 
0 
required 
0 
6 
7 
8 
Type 
I 
I 
Default 
required 
0 
  Card 2 
Variable 
Type 
Default 
1 
TB 
F 
0 
2 
TD 
F 
1021 
  VARIABLE   
DESCRIPTION
PID 
Part ID of master rigid body, see *PART. 
LCMAX 
Load curve ID defining the maximum coordinate or displacement
as a function of time.  See *DEFINE_CURVE: 
LT.0:  Load Curve ID |LCMAX| provides an upper bound for
the displacement of the rigid body 
EQ.0: no limitation of the maximum displacement. 
GT.0: Load Curve ID LCMAX provides an upper bound for the
position of the rigid body center of mass
Slave2
C.G.
Slave 1
C.G.
Master
C.G.
D1
D2
Rigid Body
Stopper
Figure 10-37.  When the master rigid body reaches the rigid body stopper, the
velocity component into the stopper is set to zero.  Slave rigid bodies 1 and 2
also stop if the distance between their mass centers and the master rigid body
is less than or equal to the input values D1 and D2, respectively. 
  VARIABLE   
LCMIN 
PSIDMX 
DESCRIPTION
Load curve ID defining the minimum coordinate or displacement
as a function of time.  See *DEFINE_CURVE: 
LT.0:  Load Curve ID |LCMIN| defines a lower bound for the
displacement of the rigid body 
EQ.0: no limitation of the minimum displacement. 
GT.0: Load  Curve  ID  LCMIN  defines  a  lower  bound  for  the
position of the rigid body center of mass 
Optional  part  set  ID  of  rigid  bodies  that  are  slaved  in  the
maximum coordinate direction to the master rigid body.  The part
set definition,  may be used to define 
the  closure  distance  (D1  and  D2  in  Figure  10-37)  which  activates 
the  constraint.    The  constraint  does  not  begin  to  act  until  the
master rigid body stops.  If the distance between the master rigid
body  is  greater  than  or  equal  to  the  closure  distance,  the  slave
rigid  body  motion  away  from  the  master  rigid  body  also  stops. 
However,  the  slaved  rigid  body  is  free  to  move  towards  the
VARIABLE   
DESCRIPTION
PSIDMN 
master.    If  the  closure  distance  is  input  as  zero  (0.0)  then  the
slaved rigid body stops when the master stops. 
Optional  part  set  ID  of  rigid  bodies  that  are  slaved  in  the 
minimum coordinate direction to the master rigid body.  The part
set definition,  may be used to define 
the  closure  distance  (D1  and  D2  in  Figure  10-37)  which  activates 
the  constraint.    The  constraint  does  not  begin  to  act  until  the
master rigid body stops.  If the distance between the master rigid
body  is  less  than  or  equal  to the  closure  distance,  the  slave  rigid
body motion towards the master rigid body also stops.  However, 
the slaved rigid body is free to move away from the master.  If the
closure  distance  is  input  as  zero  (0.0)  then  the  slaved  rigid  body
stops when the master stops. 
LCVMX 
Load curve ID which defines the maximum absolute value of the
velocity as a function of time that is allowed for the master rigid
body.  See *DEFINE_CURVE: 
EQ.0: no limitation on the velocity. 
DIR 
Direction stopper acts in: 
EQ.1: x-translation, 
EQ.2: y-translation, 
EQ.3: z-translation, 
EQ.4: arbitrary, defined by vector VID , 
EQ.5: x-axis rotation, 
EQ.6: y-axis rotation, 
EQ.7: z-axis rotation, 
EQ.8: arbitrary, defined by vector VID . 
Vector  for  arbitrary  orientation  of  stopper,  see  *DEFINE_VEC-
TOR. 
Time at which stopper is activated. 
Time at which stopper is deactivated. 
VID 
TB 
TD
Remarks: 
The  optional  definition  of  part  sets  in  minimum  or  maximum  coordinate  direction 
allows the motion to be controlled in arbitrary direction.
*CONSTRAINED_RIVET_{OPTION} 
To define an ID for the rivet, the following option is available: 
<BLANK> 
ID 
If the ID is defined an additional card is required. 
Purpose:  Define massless rivets between non-contiguous nodal pairs.  The nodes must 
not  have  the  same  coordinates.    The  action  is  such  that  the  distance  between  the  two 
nodes is kept constant throughout any motion.  No failure can be specified. 
ID Card.  Additional card for the ID keyword option.  
ID 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RID 
Type 
Default 
  Card 1 
Variable 
I 
0 
1 
N1 
Type 
I 
2 
N2 
I 
3 
TF 
F 
4 
5 
6 
7 
8 
Default 
none 
none 
1.E+20
Remarks 
1 
2 
  VARIABLE   
DESCRIPTION
RID 
N1 
N2 
Optional rivet ID. 
Node ID 
Node ID
VARIABLE   
DESCRIPTION
TF 
Failure time for nodal constraint set. 
Remarks: 
1.  Nodes  connected  by  a  rivet  cannot  be  members  of  another  constraint  set  that 
constrain  the  same  degrees-of-freedom,  a  tied  interface,  or  a  rigid  body,  i.e., 
nodes  cannot  be  subjected  to  multiple,  independent,  and  possibly  conflicting 
constraints.    Also  care  must  be  taken  to  ensure  that  single  point  constraints 
applied to nodes in a constraint set do not conflict with the constraint sets con-
strained degrees-of-freedom. 
2.  When  the  failure  time,  TF,  is  reached  the  rivet  becomes  inactive  and  the 
constrained nodes may move freely. 
Example: 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *CONSTRAINED_RIVET 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Connect node 382 to node 88471 with a massless rivet. 
$ 
*CONSTRAINED_RIVET 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$       n1        n2        tf 
       382     88471       0.0 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
*CONSTRAINED_SHELL_TO_SOLID 
Purpose:  Define a tie between a shell edge and solid elements.  Nodal rigid bodies can 
perform the same function and may also be used. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID 
NSID 
Type 
I 
I 
Default 
none 
none 
  VARIABLE   
DESCRIPTION
Shell node ID 
Solid nodal set ID, see *SET_NODE_OPTION. 
NID 
NSID 
Remarks: 
The  shell-brick  interface,  an  extension  of  the  tied  surface  capability,  ties  regions  of 
hexahedron  elements  to  regions  of  shell  elements.    A  shell  node  may  be  tied  to  up  to 
Nodes are constrained
to stay on fiber vector.
n1
n2
n3
n4
n5
s3
Nodes s1 and n3 are
coincident.
Figure 10-38.  The interface between shell elements and solids ties shell node
s1 to a line of nodes on the solid elements n1-n5.  It is very important for the
nodes to be aligned.
nine  brick  nodes  lying  along  the  tangent  vector  to  the  nodal  fiber.    See  Figure  10-38.  
During  the  calculation,  the  brick  nodes  thus  constrained,  must  lie  along  the  fiber  but 
can move relative to each other in the fiber direction.  The shell node stays on the fiber 
at the same relative spacing between the first and last brick node.  The brick nodes must 
be input in the order in which they occur, in either the plus or minus direction, as one 
moves along the shell node fiber. 
This  feature  is  intended  to  tie  four  node  shells  to  eight  node  shells  or  solids;  it  is  not 
intended for tying eight node shells to eight node solids. 
Example: 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *CONSTRAINED_SHELL_TO_SOLID 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Tie shell element, at node 329, to a solid element at node 203. 
$    - nodes 329 and 203 are coincident 
$ 
$  Additionally, define a line of nodes on the solids elements, containing 
$  node 203, that must remain in the same direction as the fiber of the shell 
$  containing node 329.  In other words: 
$ 
$    - Nodes 119, 161, 203, 245 and 287 are nodes on a solid part that 
$       define a line on that solid part. 
$    - This line of nodes will be constrained to remain linear throughout 
$       the simulation. 
$    - The direction of this line will be kept the same as the fiber of the 
$       of the shell containing node 329. 
$ 
*CONSTRAINED_SHELL_TO_SOLID 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      nid      nsid 
       329         4 
$ 
*SET_NODE_LIST 
$      sid 
         4 
$     nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
       119       161       203       245       287 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
*CONSTRAINED 
Purpose:  Define an elastic cubic spline interpolation constraint.  The displacements and 
slopes  at  the  end  points  are  continuous.    The  first  and  last  nodes,  which  define  the 
constraint,  must  be  independent.    The  degrees-of-freedom  of  interior  nodes  may  be 
either dependent or independent. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SPLID 
DLRATIO 
Type 
Default 
I 
0 
I 
0.10 
Node  Cards.    Include  one  card  per  independent/dependent  node.    The  first  and  last 
nodes must be independent.  The next “*” card terminates this input.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID 
DOF 
Type 
Default 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
SPLID 
Spline constraint ID. 
DLRATIO 
NID 
Ratio of bending to torsional stiffness for an elastic tubular beam
which connects the independent degrees-of-freedom.  The default 
value is set to 0.10. 
Independent/dependent  node  ID.    For  explicit  problems  this
node  should  not  be  a  member  of  a  rigid  body,  or  elsewhere
constrained in the input.
VARIABLE   
DOF 
DESCRIPTION
Degrees-of-freedom.    The  list  of  dependent  degrees-of-freedom 
consists  of  a  number  with  up  to  six  digits,  with  each  digit
representing  a  degree  of  freedom.    For  example,  the  value  1356 
indicates that degrees of freedom 1, 3, 5, and 6 are controlled by
the  constraint.    The  default  is  123456.    Digit:  degree  of  freedom
ID's: 
EQ.1: x 
EQ.2: y 
EQ.3: z 
EQ.4: rotation about x axis 
EQ.5: rotation about y axis 
EQ.6: rotation about z axis
*CONSTRAINED_SPOTWELD_{OPTION}_{OPTION} 
If  it  is  desired  to  use  a  time  filtered  force  calculation  for  the  forced  based  failure 
criterion then the following option is available: 
<BLANK> 
FILTERED_FORCE 
and one additional card must be defined below.  To define an ID for the spotweld the 
following option is available: 
<BLANK> 
ID 
If  the  ID  is  defined  an  additional  card  is  required.    The  ordering  of  the  options  is 
arbitrary. 
Purpose:  Define massless spot welds between non-contiguous nodal pairs. 
The  spot  weld  is  a  rigid  beam  that  connects  the  nodal  points  of  the  nodal  pairs;  thus, 
nodal rotations and displacements are coupled.  The  spot welds must be  connected to 
nodes having rotary inertias, i.e., beams or shells.  If this is not the case, for example, if 
the  nodes  belong  to  solid  elements,  use  the  option:  *CONSTRAINED_RIVET.    During 
implicit calculations this case is treated like a rivet, constraining only the displacements.  
Note  that  shell  elements  do  not  have  rotary  stiffness  in  the  normal  direction  and, 
therefore, this component cannot be transmitted. 
Spot  welded  nodes  must  not  have  the  same  coordinates.    Coincident  nodes  in  a  spot 
weld  can  be  handled  by  the  *CONSTRAINED_NODAL_RIGID_BODY  option.    Brittle 
and ductile failures are supported by this model.  Brittle failure is based on the resultant 
forces acting on the weld, and ductile failure is based on the average plastic strain value 
of  the  shell  elements  which  include  the  spot  welded  node.    Spot  welds,  which  are 
connected to massless nodes, are automatically deleted in the initialization phase and a 
warning message is printed in the messag file and the d3hsp file. 
Warning.    The  accelerations  of  spot  welded  nodes  are  output  as  zero  into  the  various 
databases,  but  if  the  acceleration  of  spotwelded  nodes  are  required,  use  either  the 
*CONSTRAINED_GENERALIZED_WELD  or  the  *CONSTRAINED_NODAL_RIGID_-
BODY input.  However, if the output interval is frequent enough accurate acceleration 
time  histories  can  be  obtained  from  the  velocity  time  history  by  differentiation  in  the 
post-processing phase.
ID Card.  Additional card for the ID keyword option. 
ID 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
WID 
Type 
Default 
  Card 1 
Variable 
I 
0 
1 
N1 
Type 
I 
2 
N2 
I 
3 
SN 
F 
4 
SS 
F 
5 
N 
F 
6 
M 
F 
7 
TF 
F 
8 
EP 
F 
Default 
none 
none  optional optional
none 
none 
1.E+20  1.E+20
Remarks 
1. 
2. 
3 
4 
Filter Card.  Additional card for the FILTERED_FORCE keyword option. 
3 
4 
5 
6 
7 
8 
  Card 2 
Variable 
1 
NF 
2 
TW 
Type 
I 
F 
Default 
none 
none 
  VARIABLE   
DESCRIPTION
WID 
Optional weld ID. 
N1 
N2 
SN 
Node ID 
Node ID 
Normal force at spotweld failure .
VARIABLE   
DESCRIPTION
Shear force at spotweld failure . 
Exponent for normal spotweld force . 
Exponent for shear spotweld force . 
Failure time for nodal constraint set. 
Effective plastic strain at failure. 
Number of force vectors stored for filtering. 
Time window for filtering. 
SS 
N 
M 
TF 
EP 
NF 
TW 
Remarks: 
1.  Nodes  connected  by  a  spot  weld  cannot  be  members  of  another  constraint  set 
that constrain the same degrees-of-freedom, a tied interface, or a rigid body, i.e., 
nodes  cannot  be  subjected  to  multiple,  independent,  and  possibly  conflicting 
constraints.    Also,  care  must  be  taken  to  ensure  that  single  point  constraints 
applied to nodes in a constraint set do not conflict with the constraint sets con-
strained degrees-of-freedom. 
2.  Failure of the spot welds occurs when: 
)
(
∣𝑓𝑛∣
𝑆𝑛
+ (
∣𝑓𝑠∣
𝑆𝑠
)
≥ 1 
where fn and fs are the normal and shear interface force.  Component fn is non-
zero for tensile values only. 
3.  When  the  failure  time,  TF,  is  reached  the  spot  weld  becomes  inactive  and  the 
constrained nodes may move freely. 
4.  Spot weld failure due to plastic straining occurs when the effective nodal plastic 
𝑝 .  This option can model the tearing out of a 
strain exceeds the input value,εfail
spotweld  from  the  sheet  metal  since  the  plasticity  is  in  the  material  that  sur-
rounds the spotweld, not the spotweld itself.  A least squares algorithm is used 
to  generate  the  nodal  values  of  plastic  strains  at  the  nodes  from  the  element 
integration  point  values.    The  plastic  strain  is  integrated  through  the  element 
and the average value is projected to the nodes via a least square fit.  This op-
tion  should  only  be  used  for  the  material  models  related  to  metallic  plasticity 
and  can  result  is  slightly  increased  run  times.    Failures  can  include  both  the 
plastic and brittle failures.
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
$$ 
$ 
$$$$  *CONSTRAINED_SPOTWELD 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
$$ 
$ 
$  Spotweld two nodes (34574 and 34383) with the approximate strength 
$  of a 3/8" SAE Grade No 3 bolt. 
$ 
*CONSTRAINED_SPOTWELD 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>...
.8 
$       n1        n2        sn        sf         n         m        tf        
ps 
     34574     34383      36.0      18.0       2.0       2.0       10.       
1.0 
$ 
$ 
$       sn = 36.0  normal failure force is 36 kN 
$       sf = 18.0  shear failure force is 18 kN 
$        n = 2.0   normal failure criteria is raised to the power of 2 
$        m = 2.0   shear failure criteria is raised to the power of 2 
$       tf = 10.0  failure occurs at time 10 unless strain failure occurs 
$       ps = 2.0   plastic strain at failure 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
$$ 
5.  Thermal:  The  2  nodes  identified  by  this  keyword  will  be  constrained  to  the 
same  temperature  in  a  thermal  problem  or  in  a  couple  thermal-mechanical 
problem.
*CONSTRAINED 
Purpose:    Define  a  self-piercing  rivet  with  failure.    This  model  for  a  self-piercing  rivet 
(SPR2)  includes  a  plastic-like  damage  model  that  reduces  the  force  and  moment 
resultants to zero as the rivet fails.  The domain of influence is specified by a diameter, 
which should be approximately equal to the rivet’s diameter. 
The location of the rivet is defined by a single node at the center of two riveted sheets.  
The  algorithm  does  a  normal  projection  from  the  master  and  slave  sheets  to  the  rivet 
node  and  locates  all  nodes  within  the  user-defined  diameter  of  influence.    The 
numerical  implementation  of  this  rivet  model  was  developed  by  L.    Olovsson  of 
Impetus Afea, based on research work on SPR point connector models originally carried 
out  by  SIMLab  (NTNU)  and  SINTEF,  see  references  by  Porcaro,  Hanssen,  and  et.al.  
[2006, 2006, 2007]. 
Originally only two sheets (master and slave) could be connected with one SPR2 node.  
But  since  release  R9,  up  to  6  sheets  can  be  connected  with  one  SPR2  by  defining 
additional  parts  on  optional  card  4.    The  following  stacking  sequence  should  be  used: 
MID – XPID1 – XPID2 – XPID3 – XPID4 – SID.  Omitted parts can be left blank, e.g.  for 
a 3-sheet connection the extra part lies in between master and slave, and for a regular 2-
sheet connection card 4 can be dropped completely.   
  Card 1 
1 
2 
3 
4 
Variable 
MID 
SID 
NSID 
THICK 
Type 
I 
I 
I 
F 
5 
D 
F 
6 
FN 
F 
7 
FT 
F 
8 
DN 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 2 
Variable 
1 
DT 
2 
XIN 
3 
4 
5 
6 
7 
8 
XIT 
ALPHA1 
ALPHA2 
ALPHA3 
DENS 
INTP 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
0.0
*CONSTRAINED_SPR2 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EXPN 
EXPT 
Type 
F 
F 
Default 
8.0 
8.0 
Card 4 is optional. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
XPID1 
XPID2 
XPID3 
XPID4 
Type 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
MID 
SID 
Master sheet Part ID 
Slave sheet Part ID 
NSID 
Node set ID of rivet location nodes. 
THICK 
Total thickness of master and slave sheet. 
D 
FN 
FT 
DN 
DT 
XIN 
XIT 
Rivet diameter. 
Rivet strength in tension (pull-out). 
Rivet strength in pure shear. 
Failure displacement in normal direction. 
Failure displacement in tangential direction. 
Fraction of failure displacement at maximum normal force. 
Fraction of failure displacement at maximum tangential force.
VARIABLE   
DESCRIPTION
ALPHA1 
Dimensionless parameter scaling the effective displacement.   
ALPHA2 
Dimensionless parameter scaling the effective displacement.   
ALPHA3 
Dimensionless parameter scaling the effective displacement.  The
sign  of  ALPHA3  can  be  used  to  choose  the  normal  update
procedure: 
GT.0: incremental update (default), 
LT.0:  total update (recommended). 
Rivet density (necessary for time step calculation). 
Flag for interpolation.  
EQ.0: linear (default),  
EQ.1: uniform, 
EQ.2: inverse distance weighting. 
Exponent value for load function in normal direction. 
Exponent value for load function in tangential direction. 
Extra part id 1 for multi-sheet connection. 
Extra part id 2 for multi-sheet connection. 
Extra part id 3 for multi-sheet connection. 
Extra part id 4 for multi-sheet connection. 
DENS 
INTP 
EXPN 
EXPT 
XPID1 
XPID2 
XPID3 
XPID4 
Self-piercing rivets are a type of fastener that is sometimes used in place of spot welds 
to join sheet metal of similar or dissimilar materials.  The rivet penetrates the first sheet, 
expands to interlock with the lower sheet without penetration.  The strength and fatigue 
characteristics  of  self-piercing  rivets  can  meet  or  even  exceed  that  of  spot  welds; 
consequently, their practical applications are expanding. 
In  the  local  description  of  the  underlying  model,  all  considerations  are  done  in  the 
plane-of-maximum opening defined by 
The unit normal vectors of the slave and master sheets are 𝐧̂𝑠 and 𝐧̂𝑚 respectively , and tangential unit normal vector of the rivet is 
𝐧̂𝑜 = 𝐧̂𝑠 × 𝐧̂𝑚. 
𝐧̂𝑡 = 𝐧̂𝑜 × 𝐧̂𝑚.
A single-sheet rivet system is assumed, i.e.  the rivet translation and rotation follow the 
motion of the master sheet.  The opening appears at the slave sheet. 
The  local  deformation  is  defined  by  normal stretch  vector δ𝑛,  tangential  stretch 𝛅𝑡  and 
total  stretch  δ = δ𝑛 + δ𝑡  .    At  any  given  time  the  total  stretch  is 
𝑠  so  that  the  scalar  measures  of  normal 
computed  from  the  position  vectors: δ = 𝐱𝑠
stretch and tangential  stretch are 𝜹𝒏 = δ ⋅ 𝐧̂𝑛 and  𝜹𝒕 = δ ⋅ 𝐧̂𝑡. The  normal and tangential 
forces  𝑓𝑛  and  𝑓𝑡  are  then  determined  by  the  material  model,  which  will  be  explained 
next. 
𝑟 − 𝐱𝑠
The moments on the rivet always satisfy, 
𝑀𝑚 + 𝑀𝑠 = (ℎ1 + ℎ2)𝑓𝑡/2. 
The motion, the forces and moments are then distributed to the nodes within the radius 
of influence by a weighting function, which is, by default, linear . 
Master Sheet (offset centerline)
Slave Sheet
Figure 10-39.  Plane of maximim opening.
Master sheet centerline
Rivet
Slave sheet centerline
Figure 10-40.  Single-sheet rivet system. 
Master sheet
Slave sheet
Figure 10-41.  Local kinematics.
Master sheet
Slave sheet
Figure 10-42.  Local forces/moments. 
The  force-deformation  relationship  is  defined  by  a  non-linear  damage  model  for 
arbitrary mixed-mode loading conditions (combination of tension and shear).  For pure 
tensile and pure shear loading, the behavior is given by, 
max𝛿𝑡
max𝛿𝑛
𝑓𝑡
𝑓𝑛
fail
fail
𝜂max𝛿𝑛
𝜂max𝛿𝑡
𝑓 ̂
𝑛(𝜂max),
𝑓 ̂
𝑡(𝜂max)
𝑓𝑛 =
𝑓𝑡 =
(1)
Respectively where, 
𝑓 ̂
𝑛(𝜂max) =
⎧
{{{
⎨
{{{
⎩
1 − (
𝜉𝑛 − 𝜂max
𝜉𝑛
EXPN
)
1 −
𝜂max − 𝜉𝑛
1 − 𝜉𝑛
   𝑓 ̂
𝑡(𝜂max) =
⎧
{{{
⎨
{{{
⎩
1 − (
𝜉𝑡 − 𝜂max
𝜉𝑡
EXPT
)
1 −
𝜂max − 𝜉𝑡
1 − 𝜉𝑡
𝜂max ≤ 𝜉𝑛
𝜂𝑚𝑎𝑥 > 𝜉𝑛
𝜂max ≤ 𝜉𝑡
𝜂𝑚𝑎𝑥 > 𝜉𝑡
(2)
In pure tension and pure shear the damage measure, 𝜂max(𝑡), defined in (3), simplifies 
to coincide with strain as indicated in figure 10-43.
Unloading
reloading path
Unloading
reloading path
Pure Tension
Pure Shear
Figure 10-43.  Force response of self penetrating rivet. 
fail  can  be  determined  directly 
max,  𝛿𝑛
Usually,  the  material  parameters  𝑓𝑛
from  experiments,  whereas  material  parameters  𝜉𝑛,  and  𝜉𝑡  can  be  found  by  reverse 
engineering.    For  mixed-mode  behavior,  an  effective  displacement  measure,  𝜂(𝜃),  is 
given by 
fail,  and  𝛿𝑡
max,  𝑓𝑡
𝜂(𝜃, 𝜂max, 𝑡 ) = [𝜉 (𝜃) +
1 − 𝜉 (𝜃)
𝛼(𝜂max)
]
√
√√
⎷
]
[
𝛿𝑛(𝑡)
fail
𝛿𝑛
+ [
]
, 
𝛿𝑡(𝑡)
fail
𝛿𝑡
(3)
where, 
𝜃 = arctan (
𝛿𝑛
𝛿𝑡
) 
𝜂max(𝑡) = max[𝜂(𝑡)]. 
The  parameter  𝜉 (𝜃)  which  ranges  from  0  to  1  scales  the  effective  displacement  as  a 
function of the direction of the displacement vector in the 𝛿𝑛-𝛿𝑡-plane according to, 
𝜉 (𝜃) = 1 −
27
(
2𝜃
)
+
27
(
2𝜃
)
.
(4)
The  directional  scaling  of  the  effective  displacement  is  allowed  to  change  as  damage 
develops, which is characterized by the shape coefficient 𝛼(𝜂max) defined as 
𝛼(𝜂max) =
⎧𝜉𝑡 − 𝜂max
{
{
𝜉𝑡
⎨
1 − 𝜂max
{
{
1 − 𝜉𝑡
⎩
𝛼1 +
𝜂max
𝜉𝑡
𝛼2
𝛼2 +
𝜂max − 𝜉𝑡
1 − 𝜉𝑡
𝜂max < 𝜉𝑡
, 
𝛼3 𝜂max ≥ 𝜉𝑡
(5)
where 𝛼1, 𝛼2, and 𝛼3 are material parameters.
Pull-out
Peeling
Isolines of
(Failure isoline)
u e l o a d i n
b li q
Shear loading
Early yielding
Figure 10-44.  Isosurfaces of 𝜂(𝜃) 
The  directional  dependency  of  the  effective  displacement  is  necessary  for  an  accurate 
force-displacement response in different loading directions.  The coefficients 𝛼1, and 𝛼2 
decrease the forces in the peeling and oblique loading cases to the correct levels.  Both 
parameters  are  usually  less  than  1;  whereas  𝛼3  is  typically  larger  than  1  as  its  main 
purpose is to moderate the failure displacement in oblique loading directions.  Several 
qualitative features captured by this model are illustrated in Figure 10-44. 
For the moment distribution, the difference between master sheet (stronger side where 
the rivet is entered) and slave sheet (weaker side) is accounted for by a gradual transfer 
from the slave to the master side as damage grows: 
𝑀𝑚 =
ℎ1 + ℎ2
(1 +
𝜂max − 𝜉1
1 − 𝜉1
) 𝑓1,
𝑀𝑠 =
ℎ1 + ℎ2
(1 −
𝜂max − 𝜉1
1 − 𝜉
) 𝑓1 
(6)
Eventually the connection to the slave sheet becomes a moment free hinge. 
It  is  recommended  to  use  the  drilling  rotation  constraint  method  for  the  connected 
components  in  explicit  analysis,  i.e.    parameter  DRCPSID  of  *CONTROL_SHELL 
should refer to all shell parts involved in SPR2 connections.
*CONSTRAINED_TIE-BREAK 
Purpose:    Define  a  tied  shell  edge  to  shell  edge  interface  that  can  release  locally  as  a 
function of plastic strain of the shells surrounding the interface nodes.  A rather ductile 
failure is achieved. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SNSID 
MNSID 
EPPF 
Type 
I 
I 
F 
Default 
none 
none 
0. 
Remarks 
1, 2 
3, 4 
  VARIABLE   
DESCRIPTION
SNSID 
Slave node set ID, see *SET_NODE_OPTION. 
MNSID 
Master node set ID, see *SET_NODE_OPTION. 
EPPF 
Plastic strain at failure 
Remarks: 
1.  Nodes  in  the  master  node  set  must  be  given  in  the  order  they  appear  as  one 
moves along the edge of the surface.   
2.  Tie-breaks may not cross. 
3.  Tie-breaks may be used to tie shell edges together with a failure criterion on the 
joint.    If  the  average  volume-weighted  effective  plastic  strain  in  the  shell  ele-
ments adjacent to a node exceeds the specified plastic strain at failure, the node 
is released.  The default plastic strain at failure is defined for the entire tie-break 
but  can  be  overridden  in  the  slave  node  set  to  define  a  unique  failure  plastic 
strain for each node. 
4.  Tie-breaks may be used to simulate the effect of failure along a predetermined 
line, such as a seam or structural joint.  When the failure criterion is reached in 
the adjoining elements, nodes along the slideline will begin to separate.  As this
effect propagates, the tie-breaks will appear to “unzip,” thus simulating failure 
of the connection.
*CONSTRAINED_TIED_NODES_FAILURE 
Purpose:  Define a tied node set with failure based on plastic strain.  The nodes must be 
coincident. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSID 
EPPF 
ETYPE 
Type 
I 
F 
Default 
none 
0. 
I 
0 
Remarks  1, 2, 3, 4 
  VARIABLE   
DESCRIPTION
NSID 
EPPF 
Nodal set ID, see *SET_NODE_OPTION. 
Plastic strain, volumetric strain, or damage (MAT_224) at failure. 
ETYPE 
Element type for nodal group: 
EQ.0: shell, 
EQ.1: solid element 
Remarks: 
1.  This feature applies to solid and shell elements using plasticity material models, 
and  to  solid  elements  using  the  honeycomb  material  *MAT_HONEYCOMB 
(EPPF = plastic  volume  strain).    The  failure  variable  is  the  volume  strain  for 
materials 26, 126, and 201.  The failure variable is the damage for material 224, 
and  the  equivalent  plastic  strain  is  used  for  all  other  plasticity  models.    The 
specified  nodes  are  tied  together  until  the  average  volume  weighted  value  of 
the  failure  variable  exceeds  the  specified  value.    Entire  regions  of  individual 
shell elements may be tied together unlike the tie-breaking shell slidelines.  The 
tied nodes are coincident until failure.  When the volume weighted average of 
the failure value is reached for a group of constrained nodes, the nodes of the 
elements that exceed the failure value are released to simulate the formation of 
a crack.
2.  To  use  this  feature  to  simulate  failure,  each  shell  element  in  the  failure  region 
should  be  generated  with  unique  node  numbers  that  are  coincident  in  space 
with  those  of  adjacent  elements.    Rather than  merging these  coincident  nodes, 
the  *CONSTRAINED_TIED_NODES_FAILURE  option  ties  the  nodal  points 
together.    As  plastic  strain  develops  and  exceeds  the  failure  strain,  cracks  will 
form and propagate through the mesh. 
3.  Entire  regions  of  individual  shell  elements  may  be  tied  together,  unlike  the 
*CONSTRAINED_TIE-BREAK  option.    This  latter  option  is  recommended 
when the location of failure is known, e.g.,  as in the plastic covers which hide 
airbags in automotive structures. 
4.  When  using  surfaces  of  shell  elements  defined  using  the  *CONSTRAINED_-
TIED_NODES_FAILURE option in contact, it is best to defined each node in the 
surface as a slave node with the NODE_TO_SURFACE contact options.  If this 
is not possible, the automatic contact algorithms beginning with *CONTACT_-
AUTOMATIC_...  all of which include thickness offsets are recommended. 
Example: 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *CONSTRAINED_TIED_NODES_FAILURE 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Tie shell elements together at the nodes specified in nodal set 101.  The 
$  constraint will be broken when the plastic strain at the nodes exceeds 0.085. 
$ 
$  In this example, four shell elements come together at a common point. 
$  The four corners of the shells are tied together with failure as opposed 
$  to the more common method of merging the nodes in the pre-processing stage. 
$ 
*CONSTRAINED_TIED_NODES_FAILURE 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$     nsid      eppf 
       101     0.085 
$ 
$ 
*SET_NODE_LIST 
$      sid 
       101 
$     nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
       775       778       896       897 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
The keyword *CONTACT provides a way of treating interaction between disjoint parts.  
Different types of contact may be defined: 
*CONTACT_OPTION1_{OPTION2}_{OPTION3}_{OPTION4}_{OPTION5} 
*CONTACT_ADD_WEAR 
*CONTACT_AUTO_MOVE 
*CONTACT_COUPLING 
*CONTACT_ENTITY 
*CONTACT_GEBOD_OPTION 
*CONTACT_GUIDED_CABLE 
*CONTACT_INTERIOR 
*CONTACT_RIGID_SURFACE 
*CONTACT_1D 
*CONTACT_2D_OPTION1_{OPTION2}_{OPTION3} 
The  first,  *CONTACT_...,  is  the  general  3D  contact  algorithms.    The  second,  *CON-
TACT_COUPLING,  provides  a  means  of  coupling  to  deformable  surfaces  to  MADY-
MO.    The  third,  *CONTACT_ENTITY,  treats  contact  using  mathematical  functions  to 
describe the surface geometry for the master surface.  The fourth, *CONTACT_GEBOD 
is  a  specialized  form  of  the  contact  entity  for  use  with  the  rigid  body  dummies  .    The  fifth,  *CONTACT_INTERIOR,  is  under  development 
and is used with soft foams where element inversion is sometimes a problem.  Contact 
between  layers  of  brick  elements  is  treated  to  eliminate  negative  volumes.    The  sixth, 
*CONTACT_RIGID_SURFACE  is  for  modeling  road  surfaces  for  durability  and  NVH 
calculations.  The seventh, *CONTACT_1D, remains in LS-DYNA for historical reasons, 
and  is  sometimes  still  used  to  model  rebars  which  run  along  edges  of  brick  elements.  
The  last,  *CONTACT_2D,  is  the  general  2D  contact  algorithm  based  on  those  used 
previously in LS-DYNA2D.
*CONTACT_OPTION1_{OPTION2}_{OPTION3}_{OPTION4}_{OPTION5}_{OPTION6} 
Purpose:    Define  a  contact  interface  in  a  3D  model.    For  contact  in  2D  models,  see 
*CONTACT_2D_OPTION. 
OPTIONS FOR *CONTACT KEYWORD 
OPTION 
REQUIRED 
DESCRIPTION 
OPTION1 
OPTION2 
OPTION3 
OPTION4 
OPTION5 
OPTION6 
Yes 
Specifies contact type 
No 
No 
No 
No 
No 
Flag for thermal 
Flag indicating ID cards follow 
Offset options 
Flag for MPP 
Flag for orthotropic friction 
Allowed values for OPTION1 
All contact types are available for explicit and implicit calculations. 
AIRBAG_SINGLE_SURFACE  
AUTOMATIC_BEAMS_TO_SURFACE 
AUTOMATIC_GENERAL 
AUTOMATIC_GENERAL_EDGEONLY 
AUTOMATIC_GENERAL_INTERIOR 
AUTOMATIC_NODES_TO_SURFACE 
AUTOMATIC_NODES_TO_SURFACE_SMOOTH 
AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE 
AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE_TIEBREAK 
AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE_SMOOTH 
AUTOMATIC_SINGLE_SURFACE  
AUTOMATIC_SINGLE_SURFACE_MORTAR
AUTOMATIC_SINGLE_SURFACE_SMOOTH 
AUTOMATIC_SINGLE_SURFACE_TIED 
AUTOMATIC_SURFACE_TO_SURFACE 
AUTOMATIC_SURFACE_TO_SURFACE_MORTAR 
AUTOMATIC_SURFACE_TO_SURFACE_MORTAR_TIED 
AUTOMATIC_SURFACE_TO_SURFACE_TIED_WELD 
AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK 
AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK_MORTAR 
AUTOMATIC_SURFACE_TO_SURFACE_SMOOTH 
CONSTRAINT_NODES_TO_SURFACE 
CONSTRAINT_SURFACE_TO_SURFACE 
DRAWBEAD 
ERODING_NODES_TO_SURFACE 
ERODING_SINGLE_SURFACE 
ERODING_SURFACE_TO_SURFACE 
FORCE_TRANSDUCER_CONSTRAINT 
FORCE_TRANSDUCER_PENALTY 
FORMING_NODES_TO_SURFACE 
FORMING_NODES_TO_SURFACE_SMOOTH 
FORMING_ONE_WAY_SURFACE_TO_SURFACE 
FORMING_SURFACE_TO_SURFACE_MORTAR 
FORMING_ONE_WAY_SURFACE_TO_SURFACE_SMOOTH 
FORMING_SURFACE_TO_SURFACE 
FORMING_SURFACE_TO_SURFACE_SMOOTH 
NODES_TO_SURFACE 
NODES_TO_SURFACE_INTERFERENCE
NODES_TO_SURFACE_SMOOTH 
ONE_WAY_SURFACE_TO_SURFACE 
ONE_WAY_SURFACE_TO_SURFACE_INTERFERENCE 
ONE_WAY_SURFACE_TO_SURFACE_SMOOTH 
RIGID_NODES_TO_RIGID_BODY 
RIGID_BODY_ONE_WAY_TO_RIGID_BODY 
RIGID_BODY_TWO_WAY_TO_RIGID_BODY 
SINGLE_EDGE 
SINGLE_SURFACE 
SLIDING_ONLY 
SLIDING_ONLY_PENALTY 
SPOTWELD 
SPOTWELD_WITH_TORSION 
SPOTWELD_WITH_TORSION_PENALTY 
SURFACE_TO_SURFACE 
SURFACE_TO_SURFACE_INTERFERENCE 
SURFACE_TO_SURFACE_SMOOTH 
SURFACE_TO_SURFACE_CONTRACTION_JOINT 
TIEBREAK_NODES_TO_SURFACE 
TIEBREAK_NODES_ONLY 
TIEBREAK_SURFACE_TO_SURFACE 
TIED_NODES_TO_SURFACE 
TIED_SHELL_EDGE_TO_SURFACE 
TIED_SHELL_EDGE_TO_SOLID 
TIED_SURFACE_TO_SURFACE 
TIED_SURFACE_TO_SURFACE_FAILURE
Allowed values for OPTION2: 
THERMAL 
THERMAL_FRICTION 
NOTE:  THERMAL  and  THERMAL_FRICTION  options  are 
restricted  to  contact  types  having  “SURFACE_TO_-
SURFACE” in OPTION1. 
Allowed value for OPTION3: 
ID 
Allowed values for OPTION4: 
OPTION4 specifies that offsets may be used with the tied contact types.  If one of these 
three offset options is set, then offsets are permitted for these contact types, and, if not, 
the nodes are projected back to the contact surface during the initialization phase and a 
constraint formulation is used.  Note that in a constraint formulation, the nodes of rigid 
bodies are not permitted in the definition. 
OFFSET 
The OFFSET option switches the formulation from a constraint type formulation 
to  one  that  is  penalty  based  where  the  force  and  moment  (if  applicable)  result-
ants  are  transferred  by  discrete  spring  elements  between  the  slave  nodes  and 
master segments. 
OFFSET is available when OPTION1 is: 
TIED_NODES_TO_SURFACE 
TIED_SHELL_EDGE_TO_SURFACE 
TIED_SURFACE_TO_SURFACE 
With  this  option,  there  is  no  coupling  between  the  transmitted  forces  and  mo-
ments  and  thus  equilibrium  is  not  enforced.    In  the  TIED_SHELL_EDGE_TO_-
SURFACE  contact,  the  BEAM_OFFSET  option  may  be  preferred  since 
corresponding  moments  accompany  transmitted  forces.    Rigid  bodies  can  be 
used with this option. 
BEAM_OFFSET
The  BEAM_OFFSET  option  switches  the  formulation  from  a  constraint  type 
formulation to one that is penalty based.  Beam-like springs are used to transfer 
force and moment resultants between the slave nodes and the master segments.  
Rigid bodies can be used with this option. 
BEAM_OFFSET is available when OPTION1 is: 
TIED_SHELL_EDGE_TO_SURFACE 
SPOTWELD 
CONSTRAINED_OFFSET 
The CONSTRAINED_OFFSET option is a constraint type formulation. 
CONSTRAINED_OFFSET is available when OPTION1 is: 
TIED_NODES_TO_SURFACE 
TIED_SHELL_EDGE_TO_SURFACE 
TIED_SURFACE_TO_SURFACE 
SPOTWELD  
Allowed value OPTION5: 
MPP 
Allowed value for OPTION6: 
ORTHO_FRICTION 
Remarks 
1.  Smooth Contact.  For SMOOTH contact, a smooth curve-fitted surface is used 
to represent the master segment, so that it can provide a more accurate repre-
sentation of the actual surface, reduce the contact noise, and produce smoother 
results  with  coarser  meshes.    All  contact  options  that  include  SMOOTH  are 
available  for  MPP.    Only  the  FORMING  contacts,  wherein  the  master  side  is 
rigid, can be used with SMOOTH in the case of SMP.
For SURFACE_TO_SURFACE and SINGLE_SURFACE contacts with SMOOTH 
in  MPP,  both  the  slave  and  master  sides  are  smoothed  every  cycle,  thereby 
slowing the contact treatment considerably.  
The SMOOTH option does not apply to segment based (SOFT = 2) contacts. 
2.  Automatic  General  Contact.    *CONTACT_AUTOMATIC_GENERAL  is  a 
single  surface  contact  similar  to  *CONTACT_AUTOMATIC_SINGLE_SUR-
FACE but which includes treatment of beam-to-beam contact and in doing so, 
checks along the entire length of the beams for penetration.  *CONTACT_AU-
TOMATIC_GENERAL essentially adds null beams to the exterior edges of shell 
parts  so  that  edge-to-edge  treatment  of  the  shell  parts  is  handled  by  virtue  of 
contact of the automatically-generated null beams.  By adding the word INTE-
RIOR  to  *CONTACT_AUTOMATIC_GENERAL,  the  contact  algorithm  goes  a 
step  further  by  adding  null  beams  to  all  the  shell  meshlines,  both  along  the 
exterior, unshared edges and the interior, shared shell edges.  The EDGEONLY 
option  skips  the  node-to-surface  contact  and  does  only  the  edge-to-edge  and 
beam-to-beam contact. 
3.  Recommendations  for  TIED  Contact  Types.    For  tying  solids-to-solids,  that 
is,  for  situations  where  none  of  the  nodes  have  rotational  degrees-of-freedom, 
use  TIED_NODES_TO_SURFACE  and  TIED_SURFACE_TO_SURFACE  type 
contacts.    These  contact  types  may  include  the  OFFSET  or  CONSTRAINED_-
OFFSET option. 
For  tying  shells-to-shells,  beams-to-shells,  that  is,  for  situations  where  all  the 
nodes  have  rotational  degrees-of-freedom,  use  TIED_SHELL_EDGE_TO_SUR-
FACE  type  contacts.    This  contact  type  may  include  the  OFFSET,  CON-
STRAINED_OFFSET, or BEAM_OFFSET option. 
TIED_SHELL_EDGE_TO_SOLID  is  intended  for  tying  shell  edges  to  solids  or 
beam  ends  to  solids,  that  is,  situations  where  only  the  slave  side  nodes  have 
rotational degrees-of-freedom. 
4.  Tied Contact Types and the Implicit Solver.  Non-physical results have been 
observed when the implicit time integrator is used for models that combine tied 
contact  formulations  with  automatic  single  point  constraints  on  solid  element 
rotational  degrees  of 
(AUTOSPC  on  *CONTROL_IMPLICIT_-
SOLVER).    The  following  subset  of  tied  interfaces  support  a  strongly  objective 
mode    and  verified  to  behave  correctly  with  the  implicit 
time integrator: 
freedom 
1)  TIED_NODES_TO_SURFACE_CONSTRAINED_OFFSET 
2)  TIED_NODES_TO_SURFACE_OFFSET
3)  TIED_SHELL_EDGE_TO_SURFACE_CONSTRAINED_OFFSET 
4)  TIED_SHELL_EDGE_TO_SURFACE_BEAM_OFFSET 
The first two of these ignore rotational degrees of freedom, while the third and 
fourth  constrain  rotations.    The  first  and  third  are  constraint  based;  while  the 
second and fourth are penalty based.  These four contact types are intended to 
cover most use scenarios. 
Setting  IACC = 1  on  *CONTROL_ACCURACY  activates  the  strongly  objective 
formulation for the above mentioned contacts (as well as the non-offset options 
*CONTACT_TIED_NODES_TO_SURFACE  and  *CONTACT_TIED_SHELL_-
EDGE_TO_SURFACE as a side effect).  When active, forces and moments trans-
form  correctly  under  superposed  rigid  body  motions  within  a  single  implicit 
step.    Additionally,  this  formulation  applies  rotational  constraints  consistently 
when, and only when, necessary.  In particular, strong objectivity is implemented 
so  that  slave  nodes  without  rotational  degrees  of  freedom  are  not  rotationally 
constrained,  while  slave  nodes  with  bending  and  torsional  rotations  are  rota-
tionally constrained.  Additionally, strong objectivity ensures that the constraint 
is physically correct. 
For a master node belonging to a shell, the slave node’s bending rotations (rota-
tions  in  the  plane  of  the  master  segment)  are  constrained  to  match  the  master 
segment’s  rotational  degrees  of  freedom;  for  master  nodes  not  belonging  to  a 
shell, the slave’s bending rotations are constrained to the master segment rota-
tion  as  determined  from  its  individual  nodal  translations.    The  slave  node’s 
torsional rotations (rotations with respect to the normal of the master segment) 
are always constrained based on the master segment’s torsional rotation as de-
termined  from  its  individual  nodal  translations,  thus  avoiding  the  relatively 
weak  drilling  mode  of  shells.    This  tied  contact  formulation  properly  treats 
bending and torsional rotations.  Since slave node rotational degrees of freedom 
typically  come  from  shell  or  beam  elements  the  most  frequently  used  options 
are: 
TIED_SHELL_EDGE_TO_SURFACE_CONSTRAINED_OFFSET 
TIED_SHELL_EDGE_TO_SURFACE_BEAM_OFFSET 
The other two “non-rotational” formulations: 
TIED_NODES_TO_SURFACE_CONSTRAINED_OFFSET 
TIED_NODES_TO_SURFACE_OFFSET 
are included for situations in which rotations do not need to be constrained at 
all.  See the LS-DYNA Theory Manual for further details.
5.  Additional  Remarks.    Additional  notes  on  contact  types  and  a  few  examples 
are provided at the end of this section in “General Remarks: *CONTACT”.   A 
theoretical discussion is provided in the LS-DYNA Theory Manual.
ADDITIONAL CARDS FOR *CONTACT KEYWORD 
Cards must appear in the exact order listed below. 
CARD 
ID 
MPP 
Card 1 
Card 2 
Card 3 
Card 4 
DESCRIPTION
Card required when OPTION3 set to ID option; otherwise 
this card is omitted. 
Card required when OPTION5 set to MPP. 
Always required. 
Always required. 
Always required. 
Required for the following permutations of *CONTACT. 
NOTE:  The  format  of  Card  4  is  different  for 
each option listed below. 
*CONTACT_AUTOMATIC_SINGLE_SURFACE_TIED
*CONTACT_CONSTRAINT_type 
*CONTACT_DRAWBEAD 
*CONTACT_ERODING_type 
*CONTACT_…_INTERFERENCE 
*CONTACT_RIGID_type 
*CONTACT_TIEBREAK_type 
*CONTACT_…_CONTRACTION_JOINT_type 
THERMAL 
Required if OPTION2 is set.  Otherwise omit. 
THERMAL_FRICTION  Required  if  OPTION2  is  set  to  THERMAL_FRICTION. 
Otherwise omit. 
ORTHO_FRICTION 
Required  if  OPTION6  is  set.    Otherwise  omit.    Contains 
friction coefficients
CARD 
DESCRIPTION
Optional Card A 
Optional parameters. 
NOTE:  Default values are highly optimized. 
NOTE:  Required  if  Optional  Card  B  is  includ-
ed.  If Optional Card A is a blank line, 
then  values  are  set  to  their  defaults, 
and Optional Card B may follow. 
Optional Card B 
Optional  parameters.    Required  if  Optional  Card  C  is 
included.  
Optional Card C 
Optional  parameters.    Required  if  Optional  Card  D  is 
included.  
Optional Card D 
Optional  parameters.    Required  if  Optional  Card  E  is 
included.  
Optional Card E 
Optional parameters.
*CONTACT_OPTION1_{OPTION2}_… 
Additional keyword for ID keyword option. 
ID 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CID 
Type 
I 
HEADING 
A70 
The  contact  ID  is  needed  during  full  deck  restarts  for  contact  initialization.    If  the 
contact  ID  is  undefined,  the  default  ID  is  determined  by  the  sequence  of  the  contact 
definitions, i.e., the first contact definition has an ID of 1, the second, 2, and so forth.  In 
a full deck restart without contact IDs, for a successful run no contact interfaces can be 
deleted  and  those  which  are  added  must  be  placed  after  the  last  definition  in  the 
previous  run.    The  ID  and  heading  is  picked  up  by  some  of  the  peripheral  LS-DYNA 
codes to aid in post-processing. 
  VARIABLE   
DESCRIPTION
CID 
Contact interface ID.  This must be a unique number. 
HEADING 
Interface  descriptor.    It  is  suggested  that  unique  descriptions  be
used.
MPP  Cards.      Variables  set  with  these  cards  are  only  active  when  using  MPP  LS-
DYNA. 
MPP Card 1.  Additional card for the MPP option.  This card is ignored, but still read 
in, when SOFT = 2 on optional card A. 
  MPP 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IGNORE 
BCKT 
LCBCKT  NS2TRK 
INITITR 
PARMAX 
CPARM8 
Type 
I 
I 
I 
Default 
0 
200 
none 
I 
3 
I 
2 
F 
See 
below 
I 
0 
MPP  Card  2.    The  keyword  reader  will  interpret  the  card  following  MPP  Card  1  as 
MPP Card 2 if the first column of the card is occupied by an ampersand.  Otherwise, it 
is  interpreted  as  Card 1.    This  card  is  ignored,  but  still  read  in,  when  SOFT = 2  on 
optional card A. 
  MPP 2 
Variable 
1 
& 
2 
3 
4 
5 
6 
7 
8 
CHKSEGS 
PENSF 
GRPABLE
Type 
Default 
I 
0 
F 
1.0 
I
IGNORE 
BCKT 
LCBCKT 
NS2TRK 
INITITR 
PARMAX 
*CONTACT_OPTION1_{OPTION2}_… 
DESCRIPTION
This is the same as the “ignore initial penetrations” option on the
*CONTROL_CONTACT Optional Card C entry 2 and can also be
specified in the normal contact control cards.  It predates both of
those,  and  is  not  really  needed  anymore  since  both  are  honored 
by  the  MPP  code.    That  is,  if  any  of  the  three  are  on,  initial
penetrations are tracked. 
Bucket  sort  frequency,  this  parameter  does  not  apply  when
SOFT = 2  on  optional  card  A  or  to  the  Mortar  contact  (option
MORTAR  on  the  CONTACT  card).    For  the  two  exceptions,  the 
BSORT option on Optional Card A applies instead. 
Load  curve  for  bucket  sort  frequency,  this  parameter  does  not
apply when SOFT = 2 on optional card A or to the Mortar contact 
(option  MORTAR  on  the  CONTACT  card). 
  For  the  two
exceptions, the negative BSORT option on Optional Card A applies 
instead. 
Number  of  potential  contacts  to  track  for  each  slave  node.    The
normal input for this (DEPTH on Optional Card A) is ignored. 
Number  of  iterations  to  perform  when  trying  to  eliminate  initial
penetrations.  Note: an input of 0 means 0, not the default value
(which is 2).  Leaving this field blank will set INITITR to 2. 
The  parametric  extension  distance  for  contact  segments.    The 
MAXPAR  parameter  on  Optional  Card  A  is  not  used  for  MPP.
For non-TIED contacts, the default is 1.0005. 
For  TIED  contacts  the  default  is  1.035  and,  the  actual  extension
used is computed as follows: 
PARMAXcomputed=
⎧1.0 + PARMAX
{{
⎨
{{
⎩
PARMAX
max(PARMAX, 1.035)
0.0 < PARMAX < 0.5
1.0 ≤ PARMAX ≤ 1.0004
otherwise
VARIABLE 
CPARM8 
CHKSEGS 
PENSF 
DESCRIPTION
Flag for CONTACT_AUTOMATIC_GENERAL behavior.  CPAR-
M8’s  value  is  interpreted  as  two  separate  flags:  OPT1  and  OPT2 
according to the rule, 
CPARM8 = OPT1 + OPT2. 
When OPT1 and OPT2 are both set, both options are active. 
OPT1: Flag to exclude beam-to-beam contact from the same PID.  
EQ.0:  Flag is not set (default). 
EQ.1:  Flag is set. 
EQ.2:  Flag  is  set.    CPARM8 = 2  has  the  additional  effect  of 
permitting  contact  treatment  of  spot  weld  (type  9)
beams 
in  AUTOMATIC_GENERAL  contacts;  spot 
weld beams are otherwise disregarded entirely by AU-
TOMATIC_GENERAL contacts. 
OPT2:  Flag to shift generated beam affecting only shell-edge-to-
shell-edge treatment.  See also SRNDE in Optional Card E. 
EQ.10:  Beam  generated  on  exterior  shell  edge  will  be  shifted
into the shell by half the shell thickness.  Therefore, the
shell-edge-to-shell-edge contact starts right at the shell 
edge and not at an extension of the shell edge. 
If this value is non-zero, then the node to surface and  surface to 
surface  contacts  will  perform  a  special  check  at  time  0  for
elements that are inverted (or nearly so), and remove them from
contact.    These  poorly  formed  elements  have  been  known  to
occur  on  the  tooling  in  metalforming  problems,  which  allows 
these  problems  to  run.    It  should  not  normally  be  needed  for
reasonable meshes. 
This  option  is  used  together  with  IGNORE  for  3D  forging
problems.    If  non-zero,  the  IGNORED  penetration  distance  is 
multiplied by this value each cycle, effectively pushing the slave 
node back out to the surface.  This is useful for nodes that might
get  generated  below  the  master  surface  during  3D  remeshing.
Care  should  be  exercised,  as  energy  may  be  generated  and
stability  may  be  effected  for  values  lower  than  0.95.    A  value  in 
the range of 0.98 to 0.99 or higher (but < 1.0) is recommended.
GRPABLE 
*CONTACT_OPTION1_{OPTION2}_… 
DESCRIPTION
Set to 1 to invoke an alternate MPP communication algorithm for
SINGLE_SURFACE, NODE_TO_SURFACE, and SURFACE_TO_-
SURFACE  contacts.    The  new  algorithm  does  not  support  all
contact  options,  including  SOFT = 2,  as  of  yet,  and  is  still  under 
development.    It  can  be  significantly  faster  and  scale  better  than
the  normal  algorithm  when  there  are  more  than  two  or  three
applicable  contact  types  defined  in  the  model.    Its  intent  is  to
speed up the contact processing but not to change the behavior of
*CONTROL_MPP_CONTACT_-
contact. 
the 
GROUPABLE. 
also 
See 
Remarks: 
1.  The MPP cards are ignored by the segment based contact options that are made 
active  by  setting  SOFT = 2  on  optional  card  A.    When  SOFT = 2.    The  BSORT 
parameter  on  optional  card  A  can  be  used  to  override  the  default  bucket  sort 
frequency.
Card 1. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
MSID 
SSTYP 
MSTYP 
SBOXID  MBOXID 
SPR 
MPR 
Type 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
I 
0 
I 
0 
Remarks 
1 
2 
optional optional  0 = off 
0 = off 
  VARIABLE   
SSID 
DESCRIPTION
Slave segment, node set ID, part set ID, part ID, or shell element 
set  ID,  see  *SET_SEGMENT,  *SET_NODE_OPTION,  *PART, 
*SET_PART or *SET_SHELL_OPTION.  For ERODING_SINGLE_-
SURFACE  and  ERODING_SURFACE_TO_SURFACE  contact 
types,  use  either  a  part  ID  or  a  part  set  ID.    For  ERODING_-
NODES_TO_SURFACE contact, use a node set which includes all
nodes that may be exposed to contact as element erosion occurs. 
EQ.0:  all  part  IDs  are  included  for  single  surface  contact,
automatic single surface, and eroding single surface. 
MSID 
Master  segment  set  ID,  part  set  ID,  part  ID,  or  shell  element  set
ID,  see  *SET_SEGMENT,  *SET_NODE_OPTION,  *PART,  *SET_-
PART, or *SET_SHELL_OPTION: 
EQ.0:  for  single  surface  contact,  automatic  single  surface,  and
eroding single surface.
VARIABLE   
DESCRIPTION
SSTYP 
ID type of SSID: 
EQ.0:  segment set ID for surface-to-surface contact, 
EQ.1:  shell element set ID for surface-to-surface contact, 
EQ.2:  part set ID, 
EQ.3:  part ID, 
EQ.4:  node set ID for node to surface contact, 
EQ.5:  include all (SSID is ignored), 
EQ.6:  part set ID for exempted parts.  All non-exempted parts 
are included in the contact. 
For  *AUTOMATIC_BEAMS_TO_SURFACE  contact  either  a  part 
set ID or a part ID can be specified. 
MSTYP 
ID type of MSID: 
EQ.0:  segment set ID, 
EQ.1:  shell element set ID, 
EQ.2:  part set ID, 
EQ.3:  part ID. 
SBOXID 
MBOXID 
EQ.4:  node  set  ID  (for  eroding  force  transducer  only.    See
remark 3),  
EQ.5:  include all (MSID is ignored). 
Include  in  contact  definition  only  those  slave  nodes/segments
within box SBOXID (corresponding to BOXID in *DEFINE_BOX), 
or    if    SBOXID  is  negative,  only  those  slave  nodes/segments
within  contact  volume  |SBOXID|  (corresponding  to  CVID  in
*DEFINE_CONTACT_VOLUME).    SBOXID  can  be  used  only  if 
SSTYP is set to 2 or 3, i.e., SSID is a part ID or part set ID.  SBOX-
ID is not available for_ERODING contact options. 
Include  in  contact  definition  only  those  master  segments  within
box  MBOXID  (corresponding  to  BOXID  in  *DEFINE_BOX),  or  if 
MBOXID  is  negative,  only  those  master  segments  within  contact
volume  |MBOXID|  (corresponding  to  CVID  in  *DEFINE_CON-
TACT_VOLUME).  MBOXID can be used only if MSTYP is set to 
2  or  3,  i.e.,  MSID  is  a  part  ID  or  part  set  ID.    MBOXID  is  not 
available for_ERODING contact options
DESCRIPTION
Include  the  slave  side  in  the  *DATABASE_NCFORC  and  the 
*DATABASE_BINARY_INTFOR 
files,  and 
optionally in the dynain file for wear: 
interface 
force 
EQ.1: slave side forces included. 
EQ.2: same  as  EQ.1,  but  also  allows  for  slave  nodes  to  be
written  as  *INITIAL_CONTACT_WEAR  to  dynain,  see
NCYC on *INTERFACE_SPRINGBACK_LSDYNA. 
Include  the  master  side  in  the  *DATABASE_NCFORC  and  the 
*DATABASE_BINARY_INTFOR 
files,  and 
optionally in the dynain file for wear: 
interface 
force 
EQ.1:  master side forces included. 
EQ.2:  same  as  EQ.1,  but  also  allows  for  master  nodes  to  be
written  as  *INITIAL_CONTACT_WEAR  to  dynain,  see 
NCYC on *INTERFACE_SPRINGBACK_LSDYNA. 
  VARIABLE   
SPR 
MPR 
Remarks: 
1.  Giving  a  slave  set  ID  equal  to  zero  is  valid  only  for  the  single  surface  contact 
algorithms, i.e., the options: 
SINGLE_SURFACE 
AUTOMATIC_… 
AIRBAG_… 
ERODING_SINGLE_SURFACE 
2.  A  master  set  ID  is  not  defined  for  the  single  surface  contact  algorithms 
(including AUTOMATIC_GENERAL).  A master set ID is optional for FORCE_-
TRANSDUCERS.    If  a  master  set  is  defined  for  the  FORCE_TRANSDUCER 
option, only those force that develop between and master and slave surfaces are 
considered.  If a transducer is  used  for extracting forces from Mortar contacts, 
the slave and master sides must be defined through parts or part sets, segment 
or node sets will not gather the correct data.
NOTE:  The  master  surface  option  of  FORCE_TRANSDUC-
ER  is  only  implemented  for  the  PENALTY  option 
and  works  only  in  conjunction  with  the  AUTO-
MATIC_SINGLE_SURFACE  contact  types,  except 
as noted in the next remark. 
3.  A master node set can only be used with the TRANSDUCER_PENALTY option, 
and requires that the slave side also be defined via a node set.  This allows the 
transducer  to  give  correct  results  for  eroding  materials.    The  node  sets  should 
include all nodes that may be exposed as erosion occurs.  This option does not 
apply to Mortar contacts.
Card 2. 
  Card 2 
Variable 
1 
FS 
Type 
F 
Default 
0. 
Remarks 
2 
FD 
F 
0. 
3 
DC 
F 
0. 
4 
VC 
F 
0. 
5 
6 
7 
VDC 
PENCHK 
BT 
8 
DT 
F 
F 
F 
0. 
I 
0 
0. 
1.0E20 
  VARIABLE   
DESCRIPTION
If OPTION1 is TIED_SURFACE_TO_SURFACE_FAILURE, then 
FS 
Normal tensile stress at failure.  failure occurs if 
[
max(0.0, 𝜎normal)
]
𝐹𝑆
+ [
𝜎shear
𝐹𝐷
]
> 1 
where  𝜎normal  and  𝜎shear  are  the  interface  normal  and  shear 
stresses. 
FD 
Shear stress at failure.  See FS. 
Else
𝜇  
𝑝3
𝑝2
𝑝1
𝑣re
Figure 11-1.  Friction coefficient,  𝜇, can be a function of relative velocity and 
pressure.  See Remarks for FS = 2.0. 
  VARIABLE   
DESCRIPTION
FS 
Static coefficient of friction.   If FS is > 0 and not equal to 2.  The 
frictional  coefficient  is  assumed  to  be  dependent  on  the  relative 
velocity 𝑣rel of the surfaces in contact according to, 
𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣. 
For mortar contact 𝜇𝑐 = FS, i.e., dynamic effects are ignored.  The 
two other possibilities are: 
EQ.-2:  If only the one friction table is defined using *DEFINE_-
FRICTION,  it  will  be  used  and  there  is  no  need  to  de-
fine  parameter  FD.    If  more  than  one  friction  table  is
defined then the Table ID is defined by the FD Parame-
ter below. 
EQ.-1:  If the frictional coefficients defined in the *PART section
are to be used, set FS to the negative number, -1.0. 
WARNING:  Please  note  that  the  FS =  -1.0  and  FS =  -2.0 
options apply only to contact types: 
SINGLE_SURFACE,  
AUTOMATIC_GENERAL,  
AUTOMATIC_SINGLE_SURFACE, 
AUTOMATIC_SINGLE_SURFACE_MORTAR,   
AUTOMATIC_NODES_TO_SURFACE,
VARIABLE   
DESCRIPTION
AUTOMATIC_SURFACE_TO_SURFACE, 
AUTOMATIC_SURFACE_TO_SURFACE_MORTAR, 
AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE, 
ERODING_SINGLE_SURFACE. 
EQ.2:  For a subset of SURFACE_TO_SURFACE type contacts 
, the variable FD serves 
as  a  table  ID  .    That  table  speci-
fies  two  or  more  values  of  contact  pressure,  with  each
pressure value in the table corresponding to a curve of
friction  coefficient  vs.    relative  velocity.    Thus  the  fric-
tion coefficient becomes a function of pressure and rela-
tive velocity.  See Figure 11-1. 
FD 
Dynamic  coefficient  of  friction.    The  frictional  coefficient  is
assumed  to  be  dependent  on  the  relative  velocity  𝑣rel  of  the 
surfaces in contact according to, 
𝜇𝑐 = FD + (FS − FD)𝑒−𝐷𝐶∣𝑣rel∣ 
For mortar contact 𝜇𝑐 = FS, i.e., dynamic effects are ignored. 
When FS = -2:   
If FS = -2 and more than one friction table is defined, FD is used
to specify friction table to be used. 
End If 
DC 
VC 
  The  frictional  coefficient  is
Exponential  decay  coefficient. 
assumed  to  be  dependent  on  the  relative  velocity  𝑣rel  of  the 
surfaces in contact 
𝜇𝑐 = FD + (FS − FD)𝑒−DC∣vrel∣. 
For mortar contact 𝜇𝑐 = FS, i.e., dynamic effects are ignored. 
Coefficient  for  viscous  friction.    This  is  necessary  to  limit  the
friction  force  to  a  maximum.    A  limiting  force  is  computed
𝐹lim = VC × 𝐴cont.    𝐴cont  being  the  area  of  the  segment  contacted 
by  the  node  in  contact.    The  suggested  value  for  VC  is  the  yield
  where  𝜎0  is  the  yield  stress  of  the 
stress  in  shear  𝑉𝐶 =
𝜎𝑜
√3
contacted material.
VDC 
*CONTACT_OPTION1_{OPTION2}_… 
DESCRIPTION
Viscous damping coefficient in percent of critical or the coefficient
of  restitution  expressed  as  percentage.    In  order  to  avoid
in  contact,  e.g.,  for  sheet  forming 
undesirable  oscillation 
simulation,  a  contact  damping  perpendicular  to  the  contacting
surfaces is applied.  When ICOR, the 6th column of the optional E 
card, is not defined or 0, the applied damping coefficient is given
by 
𝜉 =
VDC
100
𝜉crit, 
where VDC is an integer (in units of percent) between 0 and 100. 
The formula for critical damping is 
𝜉crit = 2𝑚𝜔, 
where 𝑚 is determined by nodal masses as 
𝑚 = min(𝑚slave, 𝑚master), 
and 𝜔 is determined from 𝑘, the interface stiffness, according to 
𝜔 = √𝑘
𝑚slave + 𝑚master
𝑚master𝑚slave
.
PENCHK 
Small  penetration  in  contact  search  option.    If  the  slave  node
penetrates  more  than  the  segment  thickness  times  the  factor
XPENE,  see  *CONTROL_CONTACT,  the  penetration  is  ignored 
and the slave node is set free.  The thickness is taken as the shell 
thickness if the segment belongs to a shell element or it is taken as
1/20  of  its  shortest  diagonal  if  the  segment  belongs  to  a  solid
element.    This  option  applies  to  the  surface-to-surface  contact 
algorithms:  See Table 11-17 for contact types and more details. 
BT 
Birth time (contact surface becomes active at this time). 
LT.0:  Birth  time  is  set  to  |BT|.    When  negative,  birth  time  is 
followed  during  the  dynamic  relaxation  phase  of  the
calculation.    After  dynamic  relaxation  has  completed,
contact is activated regardless the value of BT. 
EQ.0:  Birth time is inactive, i.e., contact is always active 
GT.0:  If  DT = -9999,  BT  is  interpreted  as  the  curve  or  table  ID
defining  multiple  pairs  of  birth-time/death-time,  see 
remarks below.  Otherwise, if DT > 0, birth time applies 
both during and after dynamic relaxation. 
DT 
Death time (contact surface is deactivated at this time).
VARIABLE   
DESCRIPTION
LT.0:  If  DT = -9999,  BT  is  interpreted  as  the  curve  or  table  ID
defining  multiple  pairs  of  birth-time/death-time.    Oth-
erwise,  negative  DT  indicates  that  contact  is  inactive
during  dynamic  relaxation.    After  dynamic  relaxation
the  birth  and  death  times  are  followed  and  set  to  |BT|
and |DT| respectively. 
EQ.0:  DT defaults to 1.E+20. 
GT.0:  DT, the death time, sets the time at which the contact is 
deactivated. 
Remarks: 
The  FS = 2  method  of  specifying  the  friction  coefficient  as  a  function  of  pressure  and 
relative velocity is implemented in all contacts for which SOFT = 2.  It is recommended 
that when FS = 2 and SOFT = 2 are used together, that FNLSCL be set in the range of 0.5 
to  1.0  and  DNLSCL  be  set  to  0  (refer  to  Remark  5  under  the  description  of  Optional 
Card D for *CONTACT).  If sliding is prevalent, DPRFAC = 0.01 on Optional Card C is 
also recommended. 
When FS = 2 and SOFT = 0 or 1, the following ONE_WAY contacts are recommended.  
If sliding is prevalent, DPRFAC = 0.01 is also recommended.   
ONE_WAY_SURFACE_TO_SURFACE 
(SMP and MPP) 
AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE 
(MPP only) 
FORMING_ONE_WAY_SURFACE_SURFACE_TO_SURFACE 
(MPP only) 
For SOFT = 0 or 1, FS = 2 is implemented but not advised for the following contacts: 
SURFACE_TO_SURFACE 
AUTOMATIC_SURFACE_TO_SURFACE 
FORMING_SURFACE_TO_SURFACE 
(SMP and MPP) 
(MPP only) 
(MPP only) 
A  caveat  pertaining  to  the  MPP  contacts  listed  above  is  that  the  “groupable”  option 
must not be invoked.  See *CONTROL_MPP_CONTACT_GROUPABLE.
For SOFT = 0 or 1, FS = 2 is not implemented in SMP for AUTOMATIC and FORMING  
contact types.   The static friction coefficient will literally be taken as 2.0 if FS is set to 2 
for these SMP contacts. 
If  DT = -9999,  BT  is  taken  to  be  the  ID  of  an  activation  curve  defining  multiple  birth-
times  and  death-times  as  ordered  (𝑥, 𝑦)  pairs.    A  data  point  in  the  activation  curve 
defines a time slot during which the contact is active.  For example, an activation curve 
with two data points of (20, 30) and (50, 70) activates the contact when 20 ≤ time ≤ 30 
and when 50 ≤ time ≤ 70.  To define separate activation curves for dynamic relaxation 
and  the  subsequent  dynamics,  BT  can  be  defined  as  a  table  containing  two  activation 
curves, one with VALUE = 0 for transient analysis and the other one with VALUE = 1 
for dynamic relaxation, see *DEFINE_TABLE.
Card 3. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SFS 
SFM 
SST 
MST 
SFST 
SFMT 
FSF 
VSF 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
1. 
1. 
element 
thickness
element 
thickness
1. 
1. 
1. 
1. 
  VARIABLE   
DESCRIPTION
SFS 
SFM 
SST 
MST 
SFST 
Scale  factor  on  default  slave  penalty  stiffness  when  SOFT = 0  or 
SOFT = 2, see also *CONTROL_CONTACT. 
Scale factor on default master penalty stiffness when SOFT = 0 or 
SOFT = 2, see also *CONTROL_CONTACT. 
Optional  contact  thickness  for  slave  surface  (overrides  default
contact  thickness).    This  option  applies  to  contact  with  shell  and
beam elements.  SST has no bearing on the actual thickness of the
elements;  it  only  affects  the  location  of  the  contact  surface.    For 
the  *CONTACT_TIED_…  options,  SST  and  MST  below  can  be
defined as negative values, which will cause the determination of
whether  or  not  a  node  is  tied  to  depend  only  on  the  separation
distance relative to the absolute value of these thicknesses.  More 
information  is  given  under  General  Remarks  on  *CONTACT
following Optional Card E. 
Optional  contact  thickness  for  master  surface  (overrides  default
contact thickness).  This option applies only to contact with shell
elements.    For the TIED options, see SST above. 
Scale  factor  applied  to  contact  thickness  of  slave  surface.    This
option applies to contact with shell and beam elements.  SFST has
no bearing on the actual thickness of the elements; it only affects
the  location  of  the  contact  surface.    SFST  is  ignored  if  SST  is 
nonzero  except  in  the  case  of  MORTAR  contact  .
SFMT 
FSF 
VSF 
Remarks: 
*CONTACT_OPTION1_{OPTION2}_… 
DESCRIPTION
Scale  factor  applied  to  contact  thickness  of  master  surface.    This
option applies only to contact with shell elements.  SFMT has no
bearing on the actual thickness of the elements; it only affects the
location  of  the  contact  surface.    SFMT  is  ignored  if  MST  is
nonzero  except  in  the  case  of  MORTAR  contact  . 
Coulomb  friction  scale  factor.    The  Coulomb  friction  value  is 
scaled as 𝜇𝑠𝑐 = FSF × 𝜇𝑐, see above. 
Viscous  friction  scale  factor.    If  this  factor  is  defined  then  the
limiting force becomes: 𝐹lim = VSF × VC × 𝐴cont, see above. 
The variables FSF and VSF above can be overridden segment by segment on the *SET_-
SEGMENT  or  *SET_SHELL_OPTION  cards  for  the  slave  surface  only  as  A3  and  A4, 
and for the master surface only as A1 and A2.  See *SET_SEGMENT and *SET_SHELL_
OPTION.
Card 4: AUTOMATIC_SURFACE_TIEBREAK 
This card 4 is mandatory for: 
*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK_{OPTION} 
*CONTACT_AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE_TIEBREAK_{OPTION} 
If the response parameter OPTION below is set to 9 or 11, three damping constants can 
be defined for the various failure modes.  To do this, set the keyword option to 
DAMPING 
For OPTION = 7 and OPTION = 9 but for the automatic surface to surface contact only, 
the  mortar  treatment  of  the  tiebreak  contact  may  be  activated.    This  is  primarily 
intended  for  implicit  analysis  and  no  damping  can  be  used  with  this  option,  see  also 
remarks on mortar contacts.  The keyword option for this is  
MORTAR 
The  mortar  treatment  of  tiebreak  contact  is  available  only  for  OPTION = 7  and  OP-
TION = 9, and only with surface to surface contact, i.e., neither the ONE_WAY nor the 
DAMPING option is compatible with the MORTAR option. 
  Card 4a 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OPTION 
NFLS 
SFLS 
PARAM 
ERATEN 
ERATES 
CT2CN 
CN 
Type 
I 
F 
F 
F 
F 
F 
F 
F 
Default 
required  required  required
0.0 
0.0 
0.0 
1.0 
0.0
Damping  Card.    Additional  card  for  the  case  of  OPTION = 9  with  the  DAMPING 
keyword option active. 
  Card 4b 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DMP_1 
DMP_2 
DMP_3 
Type 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
OPTION 
Response: 
EQ.-3:  see 3, moments are transferred.  SMP only. 
EQ.-2:  see 2, moments are transferred.  SMP only. 
EQ.-1:  see 1, moments are transferred.  SMP only. 
EQ.1:  slave nodes in contact and which come into contact will
permanently stick.  Tangential motion is inhibited. 
EQ.2: 
tiebreak  is  active  for  nodes  which  are  initially  in
contact.  Until failure, tangential motion is inhibited.  If
PARAM  is  set  to  unity,  (1.0)  shell  thickness  offsets  are 
ignored,  and  the  orientation  of  the  shell  surfaces  is  re-
quired such that the outward normals point to the op-
posing contact surface. 
EQ.3:  as 1 above but with failure after sticking. 
EQ.4: 
EQ.5: 
tiebreak is active for nodes which are initially in contact 
but  tangential  motion  with  frictional  sliding  is  permit-
ted. 
tiebreak  is  active  for  nodes  which  are  initially  in
contact.    Stress  is  limited  by  the  yield  condition  de-
scribed in Remark 5 below.  Damage behavior is mod-
eled  by  a  curve  which  defines  normal  stress  vs.    gap
(crack  opening).    This  option  can  be  used  to  represent
deformable glue bonds. 
EQ.6:  This option is for use with solids and thick shells only.
Tiebreak  is  active  for  nodes  which  are  initially  in  con-
tact.    Failure  stress  must  be  defined  for  tiebreak  to  oc-
cur.    After  the  failure  stress  tiebreak  criterion  is  met,
damage  is  a  linear  function  of  the  distance  C  between
VARIABLE   
DESCRIPTION
points initially in contact.  When the distance is equal to
PARAM,  damage  is  fully  developed  and  interface  fail-
ure occurs.  After failure, this option behaves as a  sur-
face-to-surface contact. 
EQ.7:  Dycoss  Discrete  Crack  Model.    “…_ONE_WAY_SUR-
FACE_TO_SURFACE_TIEBREAK”  definition  is  rec-
ommended for this option.  See Remarks. 
EQ.8:  This is similar to OPTION = 6, but it works with offset 
shell  elements.    “…_ONE_WAY_SURFACE_TO_SUR-
FACE_TIEBREAK”  definition  is  recommended  for  this 
option. 
EQ.9:  Discrete Crack Model with power law and B-K damage 
models.    “…_ONE_WAY_SURFACE_TO_SURFACE_-
TIEBREAK” definition is recommended for this option.
See Remarks. 
EQ.10:  This is similar to OPTION = 7, but it works with offset 
shell  elements.    “…_ONE_WAY_SURFACE_TO_SUR-
FACE_TIEBREAK”  definition  is  recommended  for  this 
option. 
EQ.11:  This is similar to OPTION = 9, but it works with offset 
shell  elements.    “…_ONE_WAY_SURFACE_TO_SUR-
FACE_TIEBREAK”  definition  is  recommended  for  this 
option. 
Normal failure stress for OPTION = 2, 3, 4, 6, 7, 8, 9, 10 or 11.  For 
OPTION = 5  NFLS  becomes  the  plastic  yield  stress  as  defined  in
Remark  5.    For  OPTION = 9  or  11  and  NFLS < 0,  a  load  curve 
ID = -NFLS  is  referenced  defining  normal  failure  stress  as  a
function of element size.  See remarks. 
Shear  failure  stress  for  OPTION = 2,  3,  6,  7,  8,  9,  10  or  11.    For 
OPTION = 4, SFLS is a frictional stress limit if PARAM = 1.  This 
frictional stress limit is independent of the normal force at the tie.
For  OPTION = 5  SFLS  becomes  the  curve  ID  which  defines
normal  stress  vs.    gap.    For  OPTION = 9  or  11  and  SFLS < 0,  a 
load curve ID = -SFLS is referenced defining shear failure stress as
a function of element size.  See remarks. 
NFLS 
SFLS 
PARAM 
For  OPTION =  2,  setting  PARAM = 1  causes  the  shell  thickness 
offsets  to  be  ignored.    For  OPTION = 4,  setting  PARAM = 1 
causes  SFLS  to  be  a  frictional  stress  limit.    For  OPTION = 6  or  8,
VARIABLE   
DESCRIPTION
ERATEN 
ERATES 
CT2CN 
CN 
PARAM  is  the  critical  distance,  CCRIT,  at  which  the  interface
failure is complete.  For OPTION = 7 or 10 PARAM is the friction 
angle in degrees.  For OPTION = 9 or 11, it is the exponent in the 
damage model.  A positive value invokes the power law, while a
negative one, the B-K model.  See MAT_138 for additional details.
For  OPTION =  7,  9,  10,  11  only.    Normal  energy  release  rate 
(stress ×  length)  used  in  damage  calculation,  see  Lemmen  and
Meijer [2001]. 
For OPTION = 7, 9, 10, 11 only.  Shear energy release rate (stress ×
length)  used  in  damage  calculation,  see  Lemmen  and  Meijer
[2001]. 
The  ratio  of  the  tangential  stiffness  to  the  normal  stiffness  for
OPTION = 9,  11.  The default is 1.0. 
Normal  stiffness  (stress/length)  for  OPTION =  9,  11,  and 
OPTION = 7  for  the  MORTAR  option  only.    If  CN  is  not  given
explicitly,  penalty  stiffness  divided  by  segment  area  is  used 
(default).    This  optional  stiffness  should  be  used  with  care,  since
contact  stability  can  get  affected.    A  warning  message  with  a
recommended time step is given initially. 
DMP_1 
Mode I damping force per unit velocity per unit area. 
DMP_2 
Mode II damping force per unit velocity per unit area. 
DMP_3 
Mode III damping force per unit velocity per unit area. 
Remarks: 
1.  After  failure,  this  contact  option  behaves  as  a  surface-to-surface  contact  with 
thickness offsets.  After failure, no interface tension is possible. 
2.  The  soft  constraint  option  with  SOFT = 2  is  not  implemented  for  the  tiebreak 
option. 
3.  For  OPTION = 2,  3,  and  6  the  tiebreak  failure  criterion  has  normal  and  shear 
components: 
(
|𝜎𝑛 |
NFLS
)
+ (
∣𝜎𝑠∣
SFLS
)
≥ 1.
4.  For  OPTION = 4,  the  tiebreak  failure  criterion  has  only  a  normal  stress 
component: 
|𝜎𝑛|
NFLS
≥ 1. 
5.  For OPTION = 5, the stress is limited by a perfectly plastic yield condition.  For 
ties in tension, the yield condition is 
For ties in compression, the yield condition is 
√𝜎𝑛
2 + 3∣𝜎𝑠∣2
NLFS
≤ 1. 
√3∣𝜎𝑠∣2
NLFS
≤ 1. 
The  stress  is  also  scaled  by  the  damage  function  which  is  obtained  from  the 
load curve.  For ties in tension, both normal and shear stress are scaled.  For ties 
in compression, only shear stress is scaled. 
6.  For  OPTION =   6  or  8,  damage  initiates  when  the  stress  meets  the  failure 
criterion.  The stress is then scaled by the damage function.  Assuming no load 
reversals, the energy released due to the failure of the interface is approximate-
ly 0.5 × S × CCRIT, where 
𝑆 = √max(𝜎𝑛, 0)2 + ∣𝜎𝑠∣2 
at  the  initiation  of  damage.    This  interface  may  be  used  for  simulating  crack 
propagation.  For the energy release to be correct, the contact penalty stiffness 
must be much larger than  
min(NFLF, SFLS)
. 
CCRIT
7.  OPTION = 7 or 10 is the Dycoss Discrete Crack Model as described in Lemmen 
and Meijer [2001].  The relation for the crack initiation is given as 
[
max(𝜎𝑛, 0)
NFLS
]
+ [
𝜎𝑠
SFLS − sin(PARAM)min(0, 𝜎𝑛)
]
= 1. 
8.  OPTION = 9 or 11 is based on the fracture model in the cohesive material model 
*MAT_COHESIVE_MIXED_MODE,  where  the  model  is  described  in  detail.  
Failure stresses/peak tractions NFLS and/or SFLS can be defined as functions 
of  characteristic  element  length  (square  root  of  master  segment  area)  via  load 
curve.  This option is useful to get nearly the same global responses (e.g.  load-
displacement curve) with coarse meshes compared to a fine mesh solution.  In
general, lower peak tractions are needed for coarser meshes.  See also *MAT_-
138. 
9.  For  OPTIONs  6  thru  11  of  *CONTACT_AUTOMATIC_ONE_WAY_SUR-
FACE_TO_SURFACE_TIEBREAK,  one  can  determine  the  condition  of  the  tie-
break  surface  via  the  component  labeled  "contact  gap"  in  the  intfor  database 
(*DATABASE_BINARY_INTFOR).    The  "contact  gap"  actually  represents  a 
damage value ranging from 0 (tied, no damage) to 1 (released, full damage). 
10.  Tying  in  the  AUTOMATIC_..._TIEBREAK  contacts  occurs  if  the  slave  node  is 
within a  small tolerance of the master surface after taking into account contact 
thicknesses.  For MPP, the tolerance is given by 
tol = 0.01√2 × master segment area 
for SMP, the tolerance is 0.4(slave contact thickness + master contact thickness). 
11.  It is recommended that the slave and master sides of tiebreak contact be defined 
using segment sets rather than part IDs or part set IDs.  In this way, the user can 
be  more  selective  in  choosing  which  segments  are  to  be  tied  and  ensure  that 
contact  stresses  calculated  from  nodal  contact  forces  are  not  diluted  by  seg-
ments  that  are  not  actually  on  the  actual  contact  surface.    The  user  also  has 
direct  control over  the  contact  segment  normal  vectors  when  segment  sets  are 
used.  Segment normal vectors should point toward the opposing contact sur-
face so that tension is properly distinguished from compression. 
Card 4: AUTOMATIC_SURFACE_TO_SURFACE_COMPOSITE 
This card 4 is mandatory for: 
*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_COMPOSITE 
  Card 4a 
1 
2 
3 
4 
Variable 
TFAIL 
MODEL 
CIDMU 
CIDETA 
Type 
F 
I 
I 
I 
5 
D 
F 
Default 
required  required  required required
0.0 
6 
7
VARIABLE   
DESCRIPTION
TFAIL 
Tensile traction 𝜎𝑓  required for failure. 
MODEL 
Model  for  shear  response.    See  the  equations  in  the  Remarks  for
details. 
EQ.1:  limiting shear stress depends on CIDMU in both tension
and compression.  See remark 3. 
EQ.2:  limiting shear stress depends on CIDETA in tension and
CIDMU in compression.  See remark 4. 
EQ.3:  limiting shear stress depends on CIDETA in both tension
and compression.  See remark 5. 
CIDMU 
Curve  ID  for  the  coefficient  of  friction  𝜇(𝐻)  as  a  function  of  the 
Hershey number 𝐻. 
CIDETA 
Curve ID for the viscosity 𝜂(𝑇) as a function of temperature 𝑇. 
D 
Composite film thickness. 
Remarks: 
1.  This  contact  model  is  designed  for  simulating  the  processing  of  laminated 
composite  materials.    Surfaces  in  contact  may  support  shear  up  to  the  limit 
defined by MODEL and be in compression or in tension up to the tensile limit 
𝜎𝑓  defined by TFAIL.  After TFAIL is reached, the contact fails in both tension 
and  shear.    If  the  surfaces  come  back  into  contact,  the  bonding  heals,  and  the 
contacting surfaces may support shear and tension. 
2.  The  viscosity  𝜂(𝑇)  is  defined  as  a  function  of  temperature  by  CIDETA.    The 
value of the viscosity is not extrapolated if the temperature falls outside of the 
temperature range defined by the curve. 
3.  The coefficient of friction 𝜇 for MODEL = 1 is defined in terms of the Hershey 
number  𝐻 = 𝜂(𝑇)𝑉/(𝑝 + 𝜎𝑓  ) where  p  is  the  contact  pressure  (positive  in  com-
pression, and negative in tension) and V the relative velocity between the sur-
faces. 
𝜏 ≤ μ(𝐻)(𝑝 + 𝜎𝑓 ) 
4.  The coefficient of friction 𝜇 for MODEL = 2 is defined in terms of the Hershey 
number  𝐻 = 𝜂(𝑇)𝑉/𝑝.    Note  the  definition  of  the  Hershey  number  for  this 
model differs from MODEL = 1.  In compression the shear stress is limited by 
𝜏 ≤ μ(𝐻)𝑝
and in tension, the shear stress is limited according to 
𝜏 ≤ 𝜂(𝑇)𝑉/𝑑 
5.  The  shear  stress  for  MODEL = 3  in  tension  and  compression  is  limited 
according to 
𝜏 ≤ 𝜂(𝑇)𝑉/𝑑.
Card 4: SINGLE_SURFACE_TIED 
This card 4 is mandatory for: 
*CONTACT_AUTOMATIC_SINGLE_SURFACE_TIED 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CLOSE 
Type 
F 
Default 
0.0 
  VARIABLE   
CLOSE 
Remarks: 
DESCRIPTION
Surfaces closer than CLOSE are tied.  If CLOSE is left as 0.0, it is
defaulted  to  one  percent  of  the  mesh  characteristic  length  scale.
Nodes that are above or below the surface will be tied if they are
close enough to the surface. 
This  special  feature  is  implemented  to  allow  for  the  calculation  of  eigenvalues  and 
eigenvectors on geometries that are connected by a contact interface using the AUTO-
MATIC_SINGLE_SURFACE options. 
If there is significant separation between the tied surfaces, the rigid body modes will be 
opposed by the contact stiffness, and the calculated eigenvalues for rigid body rotations 
will not be zero.
Card 4: AUTOMATIC_SURFACE_TO_SURFACE_TIED_WELD 
This card 4 is mandatory for: 
*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_TIED_WELD 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TEMP 
CLOSE 
Type 
F 
F 
Default 
None 
0.0 
DESCRIPTION
Minimum temperature required on both surfaces for tying.  Once
the  surfaces  are  tied,  they  remain  tied  even  if  the  temperature
drops. 
Surfaces closer than CLOSE are tied.  If CLOSE is left as 0.0, it is
defaulted  to  one  percent  of  the  mesh  characteristic  length  scale. 
Nodes that are above or below the surface will be tied if they are
close enough to the surface. 
  VARIABLE   
TEMP 
CLOSE 
Remarks: 
This special feature is implemented to allow for the simulation of welding.  As regions 
of the surfaces are heated to the welding temperature and come into contact, the nodes 
are tied. 
If there is significant separation between the tied surfaces, the rigid body modes will not 
be opposed by the contact stiffness.  In other words, the offset between the surfaces is 
handled like the contact with OFFSET. 
If  the  surfaces  are  below  the  welding  temperature,  the  surfaces  interact  with  the 
standard AUTOMATIC_SURFACE_TO_SURFACE options.
Card 4: CONSTRAINT_…_TO_SURFACE 
This card 4 is mandatory for: 
*CONTACT_CONSTRAINT_NODES_TO_SURFACE 
*CONTACT_CONSTRAINT_SURFACE_TO_SURFACE 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
KPF 
Type 
F 
Default 
0.0 
  VARIABLE   
DESCRIPTION
KPF 
Kinematic partition factor for constraint: 
EQ.0.0:  fully symmetric treatment. 
EQ.1.0:  one  way  treatment  with  slave  nodes  constrained  to
master  surface.    Only  the  slave  nodes  are  checked
against contact. 
EQ.-1.0:  one  way  treatment  with  master  nodes  constrained  to
slave  surface.    Only  the  master  nodes  are  checked
against contact.
Card 4: DRAWBEAD 
This card 4 is mandatory for: 
*CONTACT_DRAWBEAD 
*CONTACT_DRAWBEAD_INITIALIZE 
Note  variables  related  to  automatic  multiple  draw  bead  feature,  including  NBEAD, 
POINT1,  POINT2,  WIDTH,  and  EFFHGT  are  not  applicable  to  *CONTACT_DRAW-
BEAD_INITIALIZE. 
  Card 4a 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCIDRF 
LCIDNF 
DBDTH 
DFSCL 
NUMINT 
DBPID 
ELOFF 
NBEAD 
Type 
I 
I 
F 
F 
Default 
required  none 
0.0 
1.0 
I 
0 
I 
0 
I 
0 
I 
none 
Additional card to be included if NBEAD is defined. 
  Card 4b 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
POINT1 
POINT2  WIDTH 
EFFHGT 
Type 
I 
I 
F 
F 
Default 
none 
none 
none 
none
= Ffriction
 + Fbending
DBDTH
Figure 11-2.  The draw bead contact model. 
Initialization Card.  Additional card for INITIALIZE keyword option.  Card to initialize 
the plastic strain and thickness of elements that pass under the draw bead. 
  Card 4c 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCEPS 
TSCALE 
LCEPS2 
OFFSET 
Type 
I 
F 
I 
F 
Default 
required 
1.0 
optional optional
  VARIABLE   
LCIDRF 
LCIDNF 
DESCRIPTION
If LCIDRF is positive then it defines the load curve ID giving the
bending  component  of  the  restraining  force,  Fbending,  per  unit 
draw  bead  length  as  a  function  of  displacement,  𝛿,  see  Figure 
11-2.  This force is due to the bending and unbending of the blank 
as it moves through the draw bead.  The total restraining force is
the sum of the bending and friction components. 
If  LCIDRF  is  negative,  then  the  absolute  value  gives  the  load
curve  ID  defining  max  bead  force  versus  normalized  draw  bead 
length.    The  abscissa  values  are  between  zero  and  1  and  are  the
normalized draw bead length.  The ordinate gives the maximum
allowed draw bead, retaining force when the bead is in the fully
closed  position.    If  the  draw  bead  is  not  fully  closed,  linear 
interpolation is used to compute the draw bead force. 
Load curve ID giving the normal force per unit draw bead length
as a function of displacement, 𝛿, see Figure 11-2. 
This  force  originates  from  bending  the  blank  into  the  draw  bead 
as  the  binder  closes  on  the  die.    The  normal  force  begins  to
develop  when  the  distance  between  the  die  and  binder  is  less
than  the  draw  bead  depth.    As  the  binder  and  die  close  on  the
blank this force should diminish or reach a plateau.
DBDTH 
DFSCL 
NUMINT 
DBPID 
ELOFF 
*CONTACT_OPTION1_{OPTION2}_… 
DESCRIPTION
Draw  bead  depth,  see  Figure  11-2.    Necessary  to  determine 
correct 𝛿 displacement from contact displacements. 
Scale factor for load curve.  Default = 1.0.  This factor scales load 
curve ID, LCIDRF above. 
Number  of  equally  spaced  integration  points  along  the  draw
bead: 
EQ.0:  Internally  calculated  based  on  element  size  of  elements
that interact with draw bead. 
This  is  necessary  for  the  correct  calculation  of  the  restraining
forces.    More  integration  points  may  increase  the  accuracy  since
the force is applied more evenly along the bead. 
Optional  part  ID  for  the  automatically  generated  truss  elements
for the draw bead display in the post-processor.  If undefined LS-
DYNA assigns a unique part ID. 
Option to specify and element ID offset for the truss elements that
are  automatically  generated  for  the  draw  bead  display.    If
undefined LS-DYNA chooses a unique offset. 
NBEAD 
Number of line beads in odd integer. 
POINT1 
Node ID of the first node on a binder.  
POINT2 
Node ID of a matching node on the opposing binder. 
WIDTH 
EFFHGT 
LCEPS 
Total bead width defining distance between inner and outer most
bead walls. 
Effective bead height.  Draw bead restraining force starts to take
effect when binder gap is less than EFFHGT. 
through 
thickness. 
the  shell 
Load  curve  ID  defining  the  plastic  strain  versus  the  parametric
coordinate 
  The  parametric
coordinate  should  be  defined  in  the  interval  between  -1  and  1 
inclusive.    The  value  of  plastic  strain  at  the  integration  point  is
interpolated  from  this  load  curve.    If  the  plastic  strain  at  an
integration  point  exceeds  the  value  of  the  load  curve  at  the  time
initialization  occurs,  the  plastic  strain  at  the  point  will  remain
unchanged.
VARIABLE   
TSCALE 
LCEPS2 
DESCRIPTION
Scale factor that multiplies the shell thickness as the shell element
moves under the draw bead. 
Optional  load  curve  ID  defining  the  plastic  strain  versus  the
parametric coordinate through the shell thickness, which is  used
after  an  element  has  traveled  a  distance  equal  to  OFFSET.    The
parametric coordinate should be defined in the interval between -
1  and  1  inclusive.    The  value  of  plastic  strain  at  the  integration
point is interpolated from this load curve.  If the plastic strain at
an  integration  point  exceeds  the  value  of  the  load  curve  at  the
time  initialization  occurs,  the  plastic  strain  at  the  point  will
remain  unchanged.    Input  parameters  LCEPS2  and  OFFSET
provides a way to model the case where a material moves under
two draw beads.  In this latter case the curve would be the sum of
the  plastic  strains  generate  by  moving  under  two  consecutive
beads. 
OFFSET 
If the center of an element has moved a distance equal to OFFSET, 
the load curve ID, LCEPS2 is used to reinitialize the plastic strain.
The TSCALE scale factor is also applied. 
Overview: 
In  the  framework  of  this  draw  bead  model  the  blank  is  the  master  part,  and  the  male 
part of the draw bead is the slave.  The male part of the draw bead, which moves with 
the punch, is input as a curve defined using a list of nodes or a part consisting of beams, 
as  discussed  below.    Associated  with  this  curve  is  a  region  of  influence  that  is 
characterized by the DBDTH field of card 4a. 
As  the  punch  comes  down  and  the  region  of  influence  intersects  the  elements  on  the 
blank,  forces  are  applied  to  the  blank  at  the  points  of  closest  approach.    These  forces 
depend  on  the  separation  distance,  𝛿,  which  is  geometrically  defined  in  Figure 11-2.  
The draw bead force model consists of two terms: 
6.  There  is  a  resisting  force,  which  is  a  function  of  𝛿,  and  is  defined  through  the 
load  curve  specified  in  the  LCIDRF  field.    This  force  is  applied  in  a  direction 
opposite to velocity. 
7.  There is also a normal force pushing the male part of the draw bead away from 
the blank, which is specified by LCIDNF.  This normal force, in turn, is used to 
model friction, which depends on the product of the friction coefficient and the 
normal force.
The curve representing the male part of the draw bead can be defined in three ways: 
1.  A consecutive list of slave nodes that lie along the bead. 
2.  A part ID of a beam that lies along the draw bead. 
3.  A part set ID of beams that lie along the draw bead. 
For straight draw beads, only two nodes or a single beam needs to be defined, i.e., one 
at  each  end.    For  curved  beads,  many  nodes  or  beams  may  be  required  to  define  the 
curvature of the bead geometry. 
When beams are used to define the bead, with the exception of the first and last node, 
each  node  must  connect  with  two  beam  elements.    This  requirement  means  that  the 
number of slave nodes equals the number of beam elements plus one. 
It  is  at  the  integration  points  where  the  contact  algorithm  checks  for  penetration.  
Integration  points  are  equally  spaced  along  the  draw  bead  and  do  not  depend  on  the 
nodal spacing used in the definition of the draw bead.  By using the capability of tying 
extra  nodes  to  rigid  bodies   the draw bead nodal points do not need to belong to the 
element connectivities of the die and binder.  The blank makes up the master surface. 
NOTE: It is highly recommended to define a BOXID around 
the draw bead to limit the size of the master surface 
considered for the draw bead.  This will substantially 
reduce cost and memory requirements. 
LS-PrePost: 
While  defining  a  contact  draw  bead  may  involve  several  keywords,  the  processed  is 
streamlined by the “draw bead” definition feature of LS-PrePost4.0’s eZ-Setup for metal 
forming application.  See, 
http://ftp.lstc.com/anonymous/outgoing/lsprepost/4.0/metalforming/ 
Multiple draw beads model: 
Developed in conjunction with the Ford Motor Company Research & Advanced Engineering 
Laboratory,  the  multiple  draw  bead  features  provides  a  simple  way  to  model  (1)  the 
neglected effects of the draw bead width, and (2) to attenuate the bead forces when the 
distance between upper and lower binders is more than the draw bead height. 
1.  Draw Bead Width Correction.  As shown in Figure 11-3, it often happens that 
a sheet blank edge does not cross the draw  bead’s curve of definition but does
fall within its width.  When the bead is modelled as a 1-dimensional (no width) 
curve,  it  is  possible  that  a  major  portion  of  the  blank  would  have  no  forces 
applied, while, in reality, there are still two bending radii at the inner bead wall 
providing about 50% of the total bead forces.  The neglect of width effects leads 
to excessive blank edge draw-ins resulting in either loose metal in the part, or 
wrinkles on the draw wall or product surface. 
The multiple beads feature ameliorates this particular shortcoming by replacing 
the single 1-dimensional bead with an equivalent set of beads distributed over 
the width of the physical bead.  The bead force is distributed uniformly over the 
NBEAD sub-beads, such that the resultant force is equal to that of the original 
1-dimensionsal bead.  Note that NBEAD must be an odd integer. 
Figure  11-4  schematically  represents  the  NBEAD =  3  case  for  which  two  addi-
tional line beads are automatically generated.  The forces specified by the load 
curve,  LCIDRF,  will  be  evenly  distributed  over  the  3  beads.    In  Figure  11-5, 
bead  forces  are  recovered  from  the  ASCII  rcforc  files  for  both  cases  of 
NBEAD = 1 and 3, indicating the total force applied (shown on the left) on one 
single  bead  is  distributed  evenly  among  the  three  automatically  generated 
beads for the case of NBEAD = 3. 
The stress distribution is also more realistic with the multiple beads.  In a chan-
nel draw (half model) as shown in Figure 11-9, no significant changes in mean 
stress values are found between NBEAD = 3 and one single line bead.  In fact, 
the  compressive  stresses  are  more  realistically  and  evenly  distributed  around 
the  bead  region,  with  stresses  in  NBEAD = 3  about  1/3  of  those  in  one  line 
bead. 
2.  Lower  Binder  Gap  Correction.    As  originally  implemented,  the  draw  bead 
contact  model  applies  the  draw  bead  forces,  as  specified  in  the  load  curve, 
when the upper binder reaches the blank, regardless of the lower binder’s posi-
tion.  If the lower binder is not in contact with the blank, LS-DYNA still applies 
draw bead forces, even though it is unphysical to do so.  The EFFHGT, POINT1 
and POINT2 fields together provide a simple model to avoid these unphysical 
forces.    The  POINT1  and  POINT2  fields  are  taken  as  nodes  on  the  opposing 
binders.    The  draw  bead  contact  is  disabled  when  the  Euclidean  distance  be-
tween  POINT1  and  POINT2  is  greater  than  EFFHGT;  consequently,  the  two 
nodes must be chosen so they converge to a single point as the draw bead clos-
es. 
As shown in Figure 11-6, a simple model was built to verify the effectiveness of 
the variable EFFHGT.  The upper binder is pushed down to close with the low-
er binder while a strip of sheet blank is being pulled in the direction indicated.  
The  distance  between  the  binders  is  12mm  initially,  as  shown  in  Figure  11-7, 
and the closing gap and pulling force in x were recovered throughout the simu-
lation.    With  the  EFFHGT  set  at  8mm,  the  pulling  force  history  indicates  the 
bead forces starting to take effect after the upper binder has traveled for 4mm, 
Figure 11-8, as expected. 
Revision information: 
The NBEAD feature is available in LS-DYNA R6 Revision 69556 and later releases, with 
important updates in Revision 79270.
Inner bead wall
Blank edge flow direction
Blank drawn edge
Outer bead wall
Location of a single line bead force
Figure 11-3.  A possible scenario of sheet blank edge draw-in condition. 
Auto-created beads
Defined node set/beam
WIDTH
5.25
5.25
EFFHGT
Figure 11-4.  Definition of multiple draw beads.
)
(
14
12
10
-2
0.002
0.004
min=-7.3006
max=13559
~13559N
Legend
     rcforc bead 1
0.008
0.01
0.006
Time
)
(
-1
0.002
0.004
min=27.946
max=4523.8
~4523N
Legend
     rcforc bead 1
     rcforc bead 2
     rcforc bead 3
0.008
0.01
0.006
Time
Figure 11-5.  Bead force verification between NBEAD = 1 (left) and 3. 
Bead #3
Bead #5
Bead #4
(Beads attached to 
the upper binder)
Details in 
next figure
Figure 11-6.  A verification model for the variable EFFHGT.
POINT1(node)
Draw beads
Sheet strip
Upper binder
12mm
Tracking binder closing gap as 
abscissa values
Pull in X
Tracking the pulling force 
in X  as ordinate values
POINT2 (node) 
Lower binder
Figure 11-7. Tracking the closing gap and pulling distance. 
200
150
100
50
)
(
-50
-12
Bead force starts taking effect 
at a distance of 8.0mm
-10
-8
-6
-4
-2
Closing distance (mm)
Figure 11-8.  Pulling force (NODFOR) vs.  closure distance.
Time=0.0152, #nodes=7005, #elem=6503
Contours of pressure (mid-plane)
min=-395.339, at elem# 15423
max=28.1887, at elem# 13317
Time=0.0152, #nodes=6976, #elem=6476
Contours of pressure (mid-plane)
min=-401.24, at elem# 15280
max=74.6163, at elem# 13016
Pressure (MPa)
28.2
Pressure (MPa)
74.6
-14.2
-56.5
-98.9
-141.2
-183.6
-225.9
-268.3
-310.6
-353.0
-395.3
27.0
-20.6
-68.1
-115.7
-163.3
-210.9
-258.5
-306.1
-353.7
-401.2
Mean stresses of a channel draw 
(NBEAD=3)
Mean stresses of a channel draw 
on one line bead
Figure 11-9.  Mean stress comparison between NBEAD = 3 and 1.
Card 4: ERODING_..._SURFACE 
This card 4 is mandatory for: 
*CONTACT_ERODING_NODES_TO_SURFACE 
*CONTACT_ERODING_SINGLE_SURFACE 
*CONTACT_ERODING_SURFACE_TO_SURFACE 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ISYM 
EROSOP 
IADJ 
Type 
Default 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
ISYM 
Symmetry plane option: 
EQ.0:  off, 
EQ.1:  do  not  include  faces  with  normal  boundary  constraints
(e.g., segments of brick elements on a symmetry plane).  
This option is important to retain the correct boundary conditions
in the model with symmetry. 
EROSOP 
Erosion/Interior node option: (reset to 1 internally) 
EQ.0:  only exterior boundary information is saved, 
EQ.1:  storage  is  allocated  so  that  eroding  contact  can  occur.
Otherwise,  no  contact  is  assumed  after  erosion  of  the
corresponding element. 
IADJ 
Adjacent  material  treatment  for  solid  elements:  (reset  to  1 
internally) 
EQ.0:  solid  element  faces  are  included  only  for  free  bounda-
ries, 
EQ.1:  solid  element  faces  are  included  if  they  are  on  the
boundary of the material subset.  This option also allows
the erosion within a body and the subsequent treatment 
of contact.
*CONTACT_OPTION1_{OPTION2}_… 
Eroding contact may control the timestep .  For 
ERODING_NODES_TO_SURFACE, define the slave side using a node set, not a part ID 
or part set ID. 
Use of an ERODING contact automatically invokes a negative volume failure criterion 
in 
for  all  solid  elements 
*CONTROL_SOLID.  Use of PSFAIL will limit the negative volume failure criterion to a 
set of solid parts.  A negative volume failure criterion circumvents an error termination 
due to negative volume by deleting solid elements that develop negative volume. 
the  model,  except  as  overridden  by  PSFAIL 
in 
Contact  friction  is  not  considered  by  SMP  LS-DYNA  for  *CONTACT_ERODING_-
NODES_TO_SURFACE  and  *CONTACT_ERODING_SURFACE_TO_SURFACE  unless 
SOFT is set to 2 on Optional Card A.  MPP LS-DYNA has no such exclusion for contact 
friction. 
Values  of  EROSOP = 0  and  IADJ = 0  are  not  supported,  and  both  are  reset  to  1 
internally.
Card 4: SURFACE_INTERFERENCE 
This card 4 is mandatory for: 
*CONTACT_NODES_TO_SURFACE_INTERFERENCE 
*CONTACT_ONE_WAY_SURFACE_TO_SURFACE_INTERFERENCE 
*CONTACT_SURFACE_TO_SURFACE_INTERFERENCE 
Purpose:    This  contact  option  provides  a  means  of  modeling  parts  which  are  shrink 
fitted  together  and  are,  therefore,  prestressed  in  the  initial  configuration.    This  option 
turns off the nodal interpenetration checks (which changes the geometry by moving the 
nodes  to  eliminate  the  interpenetration)  at  the  start  of  the  simulation  and  allows  the 
contact  forces  to  develop  to  remove the  interpenetrations.    The  load  curves  defined  in 
this  section  scale  the  interface  stiffness  constants  such  that  the  stiffness  can  increase 
slowly  from  zero  to  a  final  value  with  effect  that  the  interface  forces  also  increase 
gradually to remove the overlaps. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID1 
LCID2 
Type 
Default 
I 
0 
I 
0 
DESCRIPTION
Load curve ID which scales the interface stiffness during dynamic
relaxation.    This  curve  must  originate  at  (0,  0)  at  time = 0  and 
gradually increase. 
Load  curve  ID  which  scales  the  interface  stiffness  during  the
transient calculation.  This curve generally has a constant value of 
unity  for  the  duration  of  the  calculation  if  LCID1  is  defined.    If
LCID1 = 0,  this  curve  must  originate  at  (0,  0)  at  time = 0  and 
gradually increase to a constant value. 
  VARIABLE   
LCID1 
LCID2 
Remarks: 
1.  Shell thickness offsets are taken into account for deformable shell elements.
2.  The check to fix initial penetrations is skipped. 
3.  Automatic orientation of shell elements is skipped. 
4.  Furthermore,  segment  orientation  for  shell  elements  and  interpenetration 
checks are skipped. 
Therefore, it is necessary in the problem setup to ensure that all contact segments which 
belong  to  shell  elements  are  properly  oriented,  i.e.,  the  outward  normal  vector  of  the 
segment based on the right hand rule relative to the segment numbering, must point to 
the  opposing  contact  surface;  consequently,  automatic  contact  generation  should  be 
avoided  for  parts  composed  of  shell  elements  unless  automatic  generation  is  used  on 
the slave side of a nodes to surface interface.
Card 4: RIGID_TO_RIGID 
This card 4 is mandatory for: 
*CONTACT_RIGID_NODES_TO_RIGID_BODY 
*CONTACT_RIGID_BODY_ONE_WAY_TO_RIGID_BODY 
*CONTACT_RIGID_BODY_TWO_WAY_TO_RIGID_BODY 
  Card 4 
1 
2 
Variable 
LCID 
FCM 
Type 
I 
I 
3 
US 
F 
4 
5 
6 
7 
8 
LCDC 
DSF 
UNLCID 
I 
F 
I 
Default 
required  required  LCID 
optional
0.0 
optional 
  VARIABLE   
LCID 
DESCRIPTION
Load  curve  ID  giving  force  versus  penetration  behavior  for
RIGID_contact.  See also the definition of FCM below. 
FCM 
Force calculation method for RIGID_contact: 
EQ.1:  Load  curve  gives  total  normal  force  on  surface  versus
maximum  penetration  of  any  node  (RIGID_BODY_-
ONE_WAY only). 
EQ.2:  Load  curve  gives  normal  force  on  each  node  versus
penetration  of  node  through  the  surface  (all  RIG-
ID_contact types). 
EQ.3:  Load curve gives normal pressure versus penetration of
node  through  the  surface  (RIGID_BODY_TWO_WAY 
and RIGID_BODY_ONE_WAY only). 
EQ.4:  Load  curve  gives  total  normal  force  versus  maximum
soft  penetration.    In  this  case  the  force  will  be  followed 
based  on  the  original  penetration  point.    (RIGID_-
BODY_ONE_WAY only). 
US 
Unloading  stiffness  for  RIGID_contact.    The  default  is  to  unload
along the loading curve.  This should be equal to or greater than
the maximum slope used in the loading curve.
Loading Curve
Unloading
Stiffness
Unloading Curve
Penetration
  VARIABLE   
LCDC 
Figure 11-10.  Behavior if an unloading curve is defined 
DESCRIPTION
(DC)  versus
ID  giving  damping  coefficient 
Load  curve 
penetration velocity.  The damping force FD is then: FD = DSF ×
DC × velocity. 
DSF 
Damping scaling factor. 
UNLCID 
Optional  load  curve  ID  giving  force  versus  penetration  behavior
for  RIGID_BODY_ONE_WAY  contact.    This  option  requires  the 
definition of  the unloading stiffness, US.  See Figure 11-10.
Card 4: TIEBREAK_NODES 
This card 4 is mandatory for: 
*CONTACT_TIEBREAK_NODES_TO_SURFACE and 
*CONTACT_TIEBREAK_NODES_ONLY 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NFLF 
SFLF 
NEN 
MES 
Type 
F 
F 
F 
Default 
required  required 
2. 
F 
2. 
  VARIABLE   
DESCRIPTION
Normal  failure  force.    Only  tensile  failure,  i.e.,  tensile  normal
forces, will be considered in the failure criterion. 
Shear failure force 
Exponent for normal force 
Exponent for shear force.  Failure criterion: 
(
∣𝑓𝑛∣
NFLF
NEN
)
+ (
∣𝑓𝑠∣
SFLF
MES
)
≥ 1. 
Failure is assumed if the left side is larger than 1.  𝑓𝑛 and 𝑓𝑠 are the 
normal and shear interface force. 
NFLF 
SFLF 
NEN 
MES 
Remarks: 
These attributes can be overridden node by node on the *SET_NODE_option cards. 
Both  NFLF  and  SFLF  must  be  defined.    If  failure  in  only  tension  or  shear  is  required 
then set the other failure force to a large value (1E+10). 
After  failure,  contact_tiebreak_nodes_to_surface  behaves  as  a  nodes-to-surface  contact 
with  no  thickness  offsets  (no  interface  tension  possible)  whereas  the  contact_tiebreak_
nodes_only  stops  acting  altogether.    Prior  to  failure,  the  two  contact  types  behave 
identically.
Card 4: TIEBREAK_SURFACE 
This card 4 is mandatory for: 
*CONTACT_TIEBREAK_SURFACE_TO_SURFACE and 
*CONTACT_TIEBREAK_SURFACE_TO_SURFACE_ONLY 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NFLS 
SFLS 
TBLCID 
THKOFF 
Type 
F 
F 
I 
Default 
required  required 
0 
I 
0 
  VARIABLE   
DESCRIPTION
NFLS 
SFLS 
Tensile failure stress.  See remark below. 
Shear failure stress.  Failure criterion 
(
|𝜎𝑛|
NFLS
)
+ (
)
∣𝜎𝑠∣
SFLS
≥ 1.
Optional  load  curve  number  defining  the  resisting  tensile  stress
versus  gap  opening  in  the  normal  direction  for  the  post  failure
response.    This  option  applies  only  to  SMP  and  can  be  used  to
model adhesives. 
Thickness  offsets  are  considered  if  THKOFF = 1.    If  shell  offsets 
are  included  in  the  meshed  geometry,  this  option  is  highly
recommended since segment orientation can be arbitrary and the 
contact surfaces can be disjoint.  This option is not available in the 
MPP  version  of  LS-DYNA.    It  works  by  substituting  *CON-
TACT_AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK 
(OPTION = 2  if  TBLCID  is  not  specified;  OPTION = 5  if  TBLCID 
is specified). 
TBLCID 
THKOFF 
Remarks: 
The failure attributes can be overridden segment by segment on the *SET_SEGMENT or 
*SET_SHELL_option cards for the slave surface as A1 and A2.  These variables do not 
apply  to  the  master  surface.    Both  NFLS  and  SFLS  must  be  defined.    If  failure  in  only
tension  or  shear  is  required  then  set  the  other  failure  stress  to  a  large  value  (1E+10).  
When  used  with  shells,  contact  segment  normals  are  used  to  establish  the  tension 
direction  (as  opposed  to  compression).    Compressive  stress  does  not  contribute  to  the 
failure equation. 
After failure, *CONTACT_TIEBREAK_SURFACE_TO_SURFACE behaves as a surface-
to-surface contact with no thickness offsets.   
After  failure,  *CONTACT_TIEBREAK_SURFACE_TO_SURFACE_ONLY  stops  acting 
altogether.  Until failure, it ties the slave nodes to the master nodes.
Card 4: CONTRACTION_JOINT 
This card 4 is mandatory for: 
*CONTACT_SURFACE_TO_SURFACE_CONTRACTION_JOINT 
Purpose:  This contact option turns on the contraction joint model designed to simulate 
the effects of sinusoidal joint surfaces (shear keys) in the contraction joints of arch dams 
and other concrete structures.  The  sinusoidal functions  for the shear keys are defined 
according to the following three methods [Solberg and Noble 2002]: 
Method 1: 
Method 2: 
Method 3: (default) 
𝑔̂ = 𝑔 − 𝐴{1 − cos[𝐵(𝑠2 − 𝑠1)]} 
𝑔̂ = 𝑔 − 2𝐴 ∣sin [
𝐵(𝑠2 − 𝑠1)
]∣  
𝑔̂ = 𝑔 − 𝐴cos(𝐵𝑠2) + 𝐴cos(𝐵𝑠1) 
Where 𝑔 is a gap function for contact surface, 𝑔̂ is gap function for the joint surface.  𝐴 is 
key amplitude parameter, and 𝐵 is key frequency parameter.  𝑠1 and  𝑠2 are referential 
surfaces: 
𝑠1 = 𝐗surface1 ⋅ 𝐓key 
𝑠2 = 𝐗surface2 ⋅ 𝐓key 
𝐓key = 𝐓slide × 𝐧 
Where 𝐓slide is the free sliding direction of the keys, 𝐧 is the surface normal in reference. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MTCJ 
ALPHA 
BETA 
TSVX 
TSVY 
TSVZ 
Type 
Default 
I 
0 
F 
F 
F 
F 
F 
0.0 
0.0 
0.0 
0.0 
0.0
VARIABLE   
DESCRIPTION
MTCJ 
The method option for the gap function, 𝑔̂ 
ALPHA 
Key amplitude parameter A 
BETA 
TSVX 
TSVY 
TSVZ 
Key frequency parameter B 
𝑥 component of the free sliding direction 𝐓slide 
𝑦 component of the free sliding direction 𝐓slide 
𝑧 component of the free sliding direction 𝐓slide
*CONTACT_OPTION1_{OPTION2}_… 
This card is mandatory for the THERMAL option, i.e.: 
*CONTACT_…_THERMAL_… 
Reminder:  If Card 4 is required, then it must go before this thermal card.  (Card 4 is 
required  for  certain  contact  types  -  see  earlier  in  this  section  for  the  list,  later  in  this 
section for details of Card 4.) 
Thermal Card l. 
  Card 1 
Variable 
Type 
1 
K 
F 
2 
FRAD 
F 
3 
H0 
F 
4 
5 
6 
7 
8 
LMIN 
LMAX 
FTOSLV 
BC_FLG 
ALGO 
F 
F 
F 
I 
0 
I 
0 
Default 
none 
none 
none 
none 
none 
0.5 
  VARIABLE   
DESCRIPTION
K 
Thermal  conductivity  of  fluid  between  the  contact  surfaces.    If  a
gap with a thickness 𝑙gap exists between the contact surfaces, then 
the conductance due to thermal conductivity between the contact
surfaces is 
ℎcond =
𝑙gap
Note that LS- DYNA calculates 𝑙gap based on deformation 
FRAD 
Radiation factor between the contact surfaces. 
Where, 
𝑓rad =
+ 1
𝜀2
𝜀1
− 1
𝜎 = Stefan-Boltman constant 
𝜀1 = emissivity of master surface 
𝜀2 = emissivity of slave surface 
LS-DYNA calculates a radiant heat transfer conductance 
ℎrad = 𝑓rad(𝑇𝑚 + 𝑇𝑠)(𝑇𝑚
2 + 𝑇𝑠
2)
VARIABLE   
H0 
DESCRIPTION
Heat transfer conductance for closed gaps.  Use this heat transfer
conductance for gaps in the range 
0 ≤ 𝑙gap ≤ 𝑙min
LMIN 
Minimum  gap,  𝑙min,  use  the  heat  transfer  conductance  defined 
(H0) for gap thicknesses less than this value. 
If  𝑙min < 0,  then  −𝑙min  is  a  load  curve  number  defining  𝑙min  as  a 
function time.
LMAX 
No thermal contact if gap is greater than this value (𝑙max). 
FTOSLV 
Fraction, 𝑓 ,  of  sliding  friction  energy  partitioned  to  the  slave
surface.  Energy partitioned to the master surface is (1 − 𝑓 ).  
EQ.0:  Default set to 0.5:  The 
is 
sliding 
partitioned 50% - 50% to the slave and master surfaces in 
contact. 
friction 
energy 
𝑓 =
. 
√(𝜌𝐶𝑝𝑘)
1 +
master side material
√(𝜌𝐶𝑝𝑘)
slave side material
BC_FLAG 
Thermal boundary condition flag 
EQ.0:  thermal  boundary  conditions  are  on  when  parts  are  in
contact 
EQ.1:  thermal  boundary  conditions  are  off  when  parts  are  in
contact 
ALGO 
Contact algorithm type. 
EQ.0:  two way contact, both surfaces change temperature due
to contact 
EQ.1:  one  way  contact,  master  surface  does  not  change
temperature  due  to  contact.    Slave  surface  does  change
temperature. 
Remarks: 
Note that LS- DYNA calculates 𝑙gap based on deformation
*CONTACT_OPTION1_{OPTION2}_… 
ℎ =
⎧ℎ0
{{
ℎcond + ℎrad
⎨
{{
⎩
0 ≤ 𝑙gap ≤ 𝑙min
𝑙min < 𝑙gap ≤ 𝑙max
𝑙gap > 𝑙max
THERMAL FRICTION: 
This card is required if the FRICTION suffix is added to THERMAL. 
*CONTACT_…_THERMAL_FRICTION_… 
The  blank  (or  work  piece)  must  be  defined  as  the  slave  surface  in  a  metal  forming 
model. 
Purpose: 
1.  Used  to  define  the  mechanical  static  and  dynamic  friction  coefficients  as  a 
function of temperature. 
2.  Used  to  define  the  thermal  contact  conductance  as  a  function  of  temperature 
and pressure. 
  Card 1 
1 
2 
3 
Variable 
LCFST 
LCFDT 
FORMULA
Type 
Default 
I 
0 
I 
0 
I 
0 
4 
A 
I 
0 
5 
B 
I 
0. 
6 
C 
I 
0 
7 
D 
I 
0 
8 
LCH 
I 
0 
User Subroutine Cards.  Additional cards for when FORMULA is a negative number. 
Use as many cards as necessary to set |FORMULA| number of parameters.
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
UC1 
UC2 
UC3 
UC4 
UC5 
UC6 
UC7 
UC8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
LCFST 
DESCRIPTION
Load curve number for static coefficient of friction as a function of
temperature.    The  load  curve  value  multiplies  the  coefficient
value FS.
LCFDT 
*CONTACT_OPTION1_{OPTION2}_… 
DESCRIPTION
Load  curve  number  for  dynamic  coefficient  of  friction  as  a
function  of  temperature.    The  load  curve  value  multiplies  the
coefficient value FD. 
FORMULA 
Formula that defines the contact heat conductance as a function of
temperature and pressure. 
EQ.1:  ℎ(𝑃) is defined by load curve A, which contains data for
contact conductance as a function of pressure. 
EQ.2:  ℎ(𝑃)  is  given  by  the  following  where  A,  B,  C  and  D
although  defined  by  load  curves  are  typically  constants
for use in this  formula.  The load curves are to given as 
functions of temperature. 
ℎ(𝑃) = 𝑎 + 𝑏𝑃 + 𝑐𝑃2 + 𝑑𝑃3 
EQ.3:  ℎ(𝑃) is given by the following formula from [Shvets and
Dyban 1964]. 
ℎ(𝑃) =
𝜋𝑘gas
4𝜆
[1. +85 (
0.8
)
] =
[1. +85 (
0.8
)
] 
where, 
a:  is  evaluated  from  the    load  curve,  A,  for  the  thermal
conductivity,  𝑘gas,  of  the  gas  in  the  gap  as  a  function 
of temperature. 
b:  is evaluated from the load curve, B, for the parameter
grouping 𝜋/4𝜆.  Therefore, this load curve should be 
set to a constant value.  𝜆 is the surface roughness. 
c:  is evaluated from the load curve, C , which specifies a 
stress metric for deformation (e.g., yield) as a function
of temperature. 
EQ.4:  ℎ(𝑃)  is  given  by  the  following  formula  from  [Li  and
Sellars 1996]. 
where, 
ℎ(𝑃) = 𝑎 [1 − exp (−𝑏
)]
𝑎:  is  evaluated  from  the  load  curve,  A,  which  defines  a 
load curve as a function of temperature. 
𝑏:  is  evaluated  from  the  load  curve,  B,  which  defines  a
load curve as a function of temperature.
VARIABLE   
DESCRIPTION
A 
B 
C 
D 
LCH 
𝑐:  is  evaluated  from  the  load  curve,  C,  which  defines  a
stress metric for deformation (e.g., yield) as a function 
of temperature. 
𝑑:  is  evaluated  from  the  load  curve  D,  which  is  a  func-
tion of temperature. 
EQ.5:  ℎ(gap)  is  defined  by  load  curve  A,  which  contains  data
for contact conductance as a function of interface gap. 
LT.0:  This  is  equivalent  to  defining  the  keyword  *USER_IN-
TERFACE_CONDUCTIVITY  and  the  user  subroutine 
usrhcon will be called for this contact interface for defin-
ing the contact heat transfer coefficient. 
Load curve number for the 𝑎 coefficient used in the formula. 
Load curve number for the 𝑏 coefficient used in the formula. 
Load curve number for the 𝑐 coefficient used in the formula. 
Load curve number for the 𝑑 coefficient used in the formula. 
Load curve number for ℎ.  This parameter can refer to a curve ID 
  or  a  function  ID  .    When  LCH  is  a  curve  ID  (and  a  function  ID)  it  is
interpreted as follows: 
GT.0:  the  heat  transfer  coefficient  is  defined  as  a  function  of
time, 𝑡, by a curve consisting of (𝑡, ℎ(𝑡)) data pairs. 
LT.0:  the  heat  transfer  coefficient  is  defined  as  a  function  of
temperature, 𝑇,  by  a  curve  consisting  of  (𝑇, ℎ(𝑇))  data 
pairs. 
When  the  reference  is  to  a  function  it  is  prototyped  as  follows
ℎ =  ℎ(𝑡, 𝑇avg, 𝑇slv, 𝑇msr, 𝑃, 𝑔) where: 
𝑡 = solution time 
𝑇avg = average interface temperature 
𝑇slv = slave segment temperature 
𝑇msr = master segment temperature 
𝑃 = interface pressure 
𝑔 = gap distance between master and slave segment
*CONTACT_OPTION1_{OPTION2}_… 
Additional cards for the ORTHO_FRICTION keyword option: 
*CONTACT_…_ORTHO_FRICTION_… 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FS1_S 
FD1_S 
DC1_S 
VC1_S 
LC1_S 
OACS_S 
LCFS 
LCPS 
Type 
F 
Default 
0. 
F 
0. 
F 
0. 
F 
0. 
  Card 2 
1 
2 
3 
4 
I 
0 
5 
I 
0 
6 
I 
0 
7 
I 
0 
8 
Variable 
FS2_S 
FD2_S 
DC2_S 
VC2_S 
LC2_S 
Type 
F 
Default 
0. 
  Card 3 
1 
F 
0. 
2 
F 
0. 
3 
F 
0. 
4 
I 
0 
5 
6 
7 
8 
Variable 
FS1_M 
FD1_M 
DC1_M 
VC1_M 
LC1_M  OACS_M 
LCFM 
LCPM 
Type 
F 
Default 
0. 
F 
0. 
F 
0. 
F 
0. 
I 
0 
I 
0 
I 
0 
I
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FS2_M 
FD2_M 
DC2_M 
VC2_M 
LC2_M 
Type 
F 
Default 
0. 
F 
0. 
F 
0. 
F 
0. 
I 
0 
VARIABLE 
FSn_S or M 
DESCRIPTION
Static coefficient of friction in the local n orthotropic direction for 
the  slave  (S)  or  master    (M)  surface.    The  frictional  coefficient  is
assumed  to  be  dependent  on  the  relative  velocity  𝑣rel  of  the 
surfaces in contact, 
𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣ 
where  the  direction  and  surface  are  left  off  for  clarity.    The  OR-
THO_FRICTION option applies to contact types: 
AUTOMATIC_SURFACE_TO_SUFACE, 
AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE, 
when  they  are  defined  by  segment  sets.     
specification of an offset angle in degrees from the 1-2 side which 
locates  the  1  direction.    The  offset  angle  is  input  as  the  first
attribute  of  the  segment  in  *SET_SEGMENT.    The  transverse 
direction, 2, is in the plane of the segment and is perpendicular to
the 1 direction. 
  Each  segment  in  the  set 
FDI_S or M 
Dynamic coefficient of friction in the local n orthotropic direction.
DCn_S or M 
Exponential decay coefficient for the local n direction. 
VCn_S or M 
Coefficient  for  viscous  friction  in  the  local  n  direction.    See  the 
description for VC for mandatory Card 2 above.
LCn_S or M 
*CONTACT_OPTION1_{OPTION2}_… 
DESCRIPTION
The table ID of a two dimensional table, see *DEFINE_TABLE or 
*DEFINE_TABLE_2D, giving the friction coefficient in the local n
direction  as  a  function  of  the  relative  velocity  and  interface
pressure.    In  this  case,  each  curve  in  the  table  definition  defines
the  coefficient  of 
interface  pressure 
corresponding to a particular value of the relative velocity. 
friction  versus 
the 
OACS_S or M 
LCFS or M 
If  the  default  value,  0,  is  active,  the  frictional  forces  acting  on  a
node sliding on a segment are based on the local directions of the
segment.  If OACS is set to unity, 1, the frictional forces acting on 
a  node  sliding  on  a  segment  are  based  on  the  local  directions  of
the  sliding  node.    No  matter  what  the  setting  for  OACS,  the_S 
coefficients  are  always  used  for  slave  nodes  and  the_M 
coefficients for master nodes. 
Optional  load  curve  that  gives  the  coefficient  of  friction  as  a
function  of  the  direction  of  relative  motion,  as  measured  in
degrees  from  the  first orthotropic  direction.    If  this  load  curve  is
specified, the other parameters (FS, FD, DC, VC, LC) are ignored. 
This is currently only supported in the MPP version. 
LCPS or M 
Optional  load  curve  that  gives  a  scale  factor  for  the  friction
coefficient as a function of interface pressure.  This is only used if
LCFS (or M) is defined.
Optional Card A: 
Reminder: If Card 4 is required, then it must go before this optional card.  
(Card 4 is required for certain contact types - see earlier in this section for 
the list.) 
Optional Card A. 
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SOFT 
SOFSCL 
LCIDAB  MAXPAR 
SBOPT 
DEPTH 
BSORT 
FRCFRQ 
Type 
Default 
I 
0 
F 
.1 
I 
0 
F 
F 
1.025 
0. 
I 
2 
I 
10-100 
I 
1 
Remarks 
type a13
  VARIABLE   
DESCRIPTION
SOFT 
Soft constraint option: 
EQ.0:  penalty formulation, 
EQ.1:  soft constraint formulation, 
EQ.2:  segment-based contact. 
EQ.4:  constraint approach for FORMING contact option. 
EQ.6:  special  contact  algorithm  to  handle  sheet  blank  edge
(deformable)  to  gage  pin  (rigid  shell)  contact  during
implicit  gravity  loading,  applies  to  *CONTACT_FORM-
ING_NODES_TO_SURFACE  only.    See  more  details  in 
About SOFT = 6. 
The  soft  constraint  may  be  necessary  if  the  material  constants  of
the elements which make up the surfaces in contact have a wide
variation in the elastic bulk moduli.  In the soft constraint option, 
the  interface  stiffness  is  based  on  the  nodal  mass  and  the  global
time  step  size.    This  method  of  computing  the  interface  stiffness
will  typically  give  much  higher  stiffness  value  than  would  be
obtained  by  using  the  bulk  modulus;  therefore,  this  method  the 
preferred  approach  when  soft  foam  materials  interact  with
metals.    See  the  remark  below  for  the  segment-based  penalty 
formulation.
SOFSCL 
LCIDAB 
MAXPAR 
*CONTACT_OPTION1_{OPTION2}_… 
DESCRIPTION
Scale  factor  for  constraint  forces  of  soft  constraint  option
(default=.10).  Values greater than .5 for single surface contact and 
1.0 for a one-way treatment are inadmissible. 
Load curve ID defining airbag thickness as a function of time for
type a13 contact (*CONTACT_AIRBAG_SINGLE_SURFACE). 
Maximum  parametric  coordinate  in  segment  search  (values 
between 1.025 and 1.20 are recommended).  This variable applies
only to SMP; for MPP, see PARMAX.  Larger values can increase
cost.    If  zero,  the  default  is  set  to  1.025  for  most  contact  options.
Other defaults are: 
EQ.1.006:  SPOTWELD, 
EQ.1.006:  TIED_SHELL_…_CONSTRAINED_OFFSET, 
EQ.1.006:  TIED_SHELL_…_OFFSET, 
EQ.1.006:  TIED_SHELL_…_:BEAM_OFFSET, 
EQ.1.100:  AUTOMATIC_GENERAL 
This  factor  allows  an  increase  in  the  size  of  the  segments  which
may  be  useful  at  sharp  corners.      For  the  SPOTWELD  and  …_
OFFSET  options  larger  values  can  sometimes  lead  to  numerical
instabilities;  however,  a  larger  value  is  sometimes  necessary  to
ensure that all nodes of interest are tied. 
SBOPT 
Segment-based contact options (SOFT = 2). 
EQ.0:  defaults to 2. 
EQ.1:  pinball edge-edge contact  (not recommended) 
EQ.2:  assume planer segments (default) 
EQ.3:  warped segment checking 
EQ.4:  sliding option 
EQ.5:  do options 3 and 4
VARIABLE   
DEPTH 
BSORT 
FRCFRQ 
DESCRIPTION
Search  depth  in  automatic  contact,  check  for  nodal  penetration
through the closest contact segments.  Value of 1 (one segment) is
sufficiently accurate for most crash applications and is much less
expensive.  LS-DYNA for improved accuracy sets this value to 2 
(two segments), which is default when set to zero, default search
depth for *CONTACT_AUTOMATIC_GENERAL is 3. 
LT.0:  |DEPTH| is the load curve ID defining searching depth
versus time.  (not available when SOFT = 2) 
See remarks below for segment-based contact (SOFT = 2)  
options controlled by DEPTH. 
Number of cycles between bucket sorts.  Values of 25 and 100 are
recommended  for  contact  types  4  and  13  (SINGLE_SURFACE), 
respectively.    Values  of  10-15  are  okay  for  the  surface  to  surface 
and  node  to  surface  contact.    If  zero,  LS-DYNA  determines  the 
interval.  BSORT applies only to SMP   except  in  the  case  of  SOFT = 2  or  for  Mortar  contact 
(option MORTAR on the CONTACT card), in which case BSORT 
applies to both SMP and MPP.  For Mortar contact the default is
the value associated with NSBCS on *CONTROL_CONTACT. 
LT.0:  |BSORT| 
load  curve 
ID  defining  bucket  sorting
frequency versus time. 
Number  of  cycles  between  contact  force  updates  for  penalty
contact  formulations.    This  option  can  provide  a  significant
speed-up of the contact treatment.  If used, values exceeding 3 or
4  are  dangerous.    Considerable  care  must  be  exercised  when
using  this  option,  as  this  option  assumes  that  contact  does  not
change FRCFRG cycles. 
EQ.0:  FRCFRG is set to 1 and force calculations are performed
each cycle-strongly recommended.
Nodes in NSET #21 (create 
'by path' in LSPP4.0)
Sheet blank
Sheet blank
Fixed in XZ
Gage pin (PID 20)
Fixed in Z
Fixed in XZ
Gravity loading in -Y
Gage pin
Binder ring
Lower post
Figure  11-11.    Illustrative/test  model  for  SOFT = 6  (left)  and  initial  blank
position. 
General remarks: 
Setting  SOFT = 1  or  2  on  optional  contact  card  A  will  cause  the  contact  stiffness  to  be 
determined  based  on  stability  considerations,  taking  into  account  the  time  step  and 
nodal masses.  This approach is generally more effective for contact between materials 
of dissimilar stiffness or dissimilar mesh densities. 
About SOFT = 2: 
SOFT = 2  is  for  general  shell  and  solid  element  contact.    This  option  is  available  for 
SURFACE_TO_SURFACE,  ONE_WAY_SURFACE_TO_SURFACE,  and  SINGLE_SUR-
FACE  options  including  AUTOMATIC,  ERODING,  and  AIRBAG  contact.    When  the 
AUTOMATIC option is used, orientation of shell segment normals is automatic.  When 
the  AUTOMATIC  option  is  not  used,  the  segment  or  element  orientations  are  used  as 
input.    The  segment-based  penalty  formulation  contact  algorithm  checks  for  segments 
vs.  segment penetration rather than node vs.  segment.  After penetrating segments are 
found, an automatic judgment is made as to which is the master segment, and penalty 
forces  are  applied  normal  to  that  segment.    The  user  may  override  this  automatic 
judgment by using the ONE_WAY options in which case the master segment normals 
are used as input by the user.  All parameters on the first three cards are active except 
for VC, and VSF.  On optional card A, some parameters have different meanings than 
they do for the default contact. 
For  SOFT = 2,  the  SBOPT  parameter  on  optional  card  A  controls  several  options.  
Setting  DEPTH = 1  for  pinball  edge-to-edge  checking  is  not  recommended  and  is
included only for back compatibility.  For edge-to-edge checking setting DEPTH = 5 is 
recommended instead .  The warped segment option more accurately checks 
for  penetration  of  warped  surfaces.    The  sliding  option  uses  neighbor  segment 
information to improve sliding behavior.  It is primarily useful for preventing segments 
from incorrectly catching nodes on a sliding surface. 
For  SOFT = 2,  the  DEPTH  parameter  controls  several  additional  options  for  segment 
based contact. 
1.  DEPTH =  2  (former  default;  not  recommended).    surface  penetrations 
measured at nodes are checked. 
2.  DEPTH =  3  (current  default).    Surface  penetration  is  also  be  measured  at  the 
edge.    This  option  is  more  accurate  than  DEPTH=2,  and  is  good  for  a  wide 
variety of simulations, but does not check for edge-to-edge penetration. 
3.  DEPTH =  5.    Both  surface  penetrations  and  edge-to-edge  penetration  is 
checked. 
4.  DEPTH =  13.    The  penetration  checking  is  the  same  as  for  DEPTH=3,  but  the 
code has been tuned to better conserve energy. 
5.  DEPTH = 23 or 33.  The penetration checking is similar to DEPTH=3, but new 
methods are used to try to improve robustness. 
6.  DEPTH =  25  or  35.    The  penetration  checking  is  similar  to  DEPTH=5  but  use 
new methods to try to improve robustness. 
7.  DEPTH = 45. The splitting pinball method [Belytschko and Yeh, 1993] is used.  
This method is more accurate at the cost of more CPU time, and is recommend-
ed when modeling complex contacts between parts comprised of shells.  It does 
not  apply  to  solid  or  thick  shell  parts  but  such  parts  can  be  coated  with  null 
shells as a means of making DEPTH=45 available. 
8.  DEPTH = 1 or 4.  The airbag contact has two additional options, DEPTH=1 and 
4.    DEPTH=4  activates  additional  airbag  logic  that  uses  neighbor  segment  in-
formation when judging if contact is between interior or exterior airbag surfac-
es.    This  option  is  not  recommended  and  is  maintained  only  for  backward 
compatibility.  Setting DEPTH=1 suppresses all airbag logic. 
For  SOFT = 2  contact,  only  the  ISYM,  I2D3D,  SLDTHK,  and  SLDSTF  parameters  are 
active on optional card B.  Also, the negative MAXPAR option is now incorporated into 
the  DTSTIF  option  on  optional  card  C.    Data  that  uses  the  negative  MAXPAR  option 
will continue to run correctly.
Binder ring
Pin / blank edge 
contact enforced
Lower post
Gage pin
Sheet blank 
final position
Sheet blank 
final position
Gravity loading results without using 
SOFT=6; Pin/blank edge contact missed.
Gravity loading results using SOFT=6; 
Pin/blank edge contact sucessful.
  Figure 11-12.  Final blank position without (left) and with (right) SOFT = 6. 
About SOFT = 6: 
SOFT = 6  contact  addresses  contact  issues  in  situation  where  blank  gage  pins  are 
narrow  or  small  and  blank  mesh  are  coarse  (Figure  11-11  left),  leading  to  missing 
contact in some cases.  This feature applies only to gravity loading of sheet blank with 
non-adaptive  mesh,  and  for  use  with  *CONTACT_FORMING_NODES_TO_SUR-
FACE only. 
set 
for 
included 
in  a  node 
the  variable  SSID 
Nodes  along  the  entire  or  a  portion  of  the  blank  edge  to  be  contacted  with  gage  pins 
*  CON-
must  be 
TACT_FORMING_NODES_TO_SURFACE  (Figure  11-11  left).    The  nodes  in  the  node 
set must be listed in a consecutive order, as defined “by path” in LSPP4.0, under Model 
→ CreEnt → Cre → Set Data → *SET_NODE.  No thickness exists for either blank edge or 
gage pins.  In addition, the variable ORIENT in *CONTROL_CONTACT must be set to 
“4”.    Currently  this  feature  is  available  in  double  precision,  SMP  only,  starting  in 
in 
Revision  81297  and 
*CONTACT_FORMING_NODES_TO_SURFACE  can  be  input  as  part  ID  of  the  blank, 
making it much easier to use SOFT = 6. 
in  Revision  110072,  SSID 
later  releases. 
  Starting 
in
In a partial keyword example below, node set ID 21 (SSTYP = 4) is in contact with gage 
pin  of  part  set  ID  20.    As  shown  in  Figure  11-11  (left),  with  the  boundary  condition 
applied, a blank with a very coarse mesh is loaded with a body force.  The left notch is 
anticipated to be in contact with the gage pins.  The initial position (top view) of the test 
model is shown in Figure 11-11 (right) and the final gravity loaded blank positions are 
shown  in  Figure  11-12  (left)  without  SOFT = 6,  and  in  Figure  11-12  (middle  and  right) 
with SOFT = 6, respectively.  It is shown that without the SOFT = 6 the contact between 
the blank edge and the pin missed completely. 
*CONTROL_TERMINATION 
1.0 
*CONTROL_IMPLICIT_FORMING 
1 
*CONTROL_IMPLICIT_GENERAL 
1,0.2 
*CONTROL_IMPLICIT_NONLINEAR 
$  NSLOLVR    ILIMIT    MAXREF     DCTOL     ECTOL     RCTOL     LSTOL 
         2         1      1200     0.000      0.00         0 
$    dnorm   divflag   inistif 
         0         2         0        1                  1 
*SET_NODE_LIST 
$ blank edge node set around the gage pin 
21 
1341,1342,1343,1344 
*SET_PART_LIST 
$ gage pin 
20 
20 
*SET_PART_LIST 
$ blank 
13 
13 
*CONTACT_FORMING_NODES_TO_SURFACE 
$     SSID      MSID     SSTYP     MSTYP    SBOXID    MBOXID       SPR       MPR 
        21        20         4         2 
$       FS        FD        DC         V       VDC    PENCHK        BT        DT 
     0.125                                     20.         4 
$      SFS       SFM       SST       MST      SFST      SFMT       FSF       VSF 
$     SOFT 
         6 
Beginning in Revision109342, an SSTYP of 3 (a part PID, not a part set ID) can be used 
for  the  SSID,  simplifying  the  definition  of  contact  interfaces  for  SOFT = 6.    In  Soft  6 
contact definition below, a blank PID of 13 is defined for the SSID using SSTYP = 3: 
*CONTACT_FORMING_NODES_TO_SURFACE 
$     SSID      MSID     SSTYP     MSTYP    SBOXID    MBOXID       SPR       MPR 
        13        20         3         2 
$       FS        FD        DC         V       VDC    PENCHK        BT        DT 
     0.125                                     20.         4 
$      SFS       SFM       SST       MST      SFST      SFMT       FSF       VSF 
$     SOFT 
         6

Optional Card B: 
Reminder:  If Optional Card B is used, then Optional Card A must be defined.  
(Optional Card A may be a blank line). 
Optional Card B. 
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PENMAX 
THKOPT 
SHLTHK 
SNLOG 
ISYM 
I2D3D 
SLDTHK 
SLDSTF 
Type 
Default 
F 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
F 
0 
F 
0 
Remarks 
  VARIABLE   
PENMAX 
Old 
types 3, 
5, 10 
Old 
types 3, 
5, 10 
DESCRIPTION
Maximum  penetration  distance  for  old  type  3,  5,  8,  9,  10  and
Mortar contact or the segment thickness multiplied by PENMAX
defines  the  maximum  penetration  allowed  (as  a  multiple  of  the
segment  thickness)  for contact  types  a  3,  a  5,  a10,  13,  15,  and  26.
: 
EQ.0.0:  for old type contacts 3, 5, and 10: Use small penetration
search  and  value  calculated  from  thickness  and
XPENE, see *CONTROL_CONTACT. 
EQ.0.0:  for contact types a 3, a 5, a10, 13, and 15: Default is 0.4, 
or 40 percent of the segment thickness 
EQ.0.0:  for  contact  type26  the  default  value  is  the  segment
thickness multiplied by 10 
EQ.0.0: for Mortar contact the default is a characteristic size of
the element, see Theory manual
VARIABLE   
DESCRIPTION
THKOPT 
Thickness option for contact types 3, 5, and 10: 
SHLTHK 
EQ.0:  default  is  taken  from  control  card,  *CONTROL_CON-
TACT, 
EQ.1:  thickness offsets are included, 
EQ.2:  thickness offsets are not included (old way). 
Define  if  and  only  if  THKOPT  above  equals  1.    Shell  thickness 
considered  in  type  surface  to  surface  and  node  to  surface  type
contact  options,  where  options  1  and  2  below  activate  the  new
contact  algorithms.    The  thickness  offsets  are  always  included  in
single surface and constraint method contact types: 
EQ.0:  thickness is not considered, 
EQ.1:  thickness is considered but rigid bodies are excluded, 
EQ.2:  thickness is considered including rigid bodies. 
SNLOG 
Disable shooting node logic in thickness offset contact.  With the
shooting  node  logic  enabled,  the  first  cycle  that  a  slave  node
penetrates  a  master  segment,  that  node  is  moved  back  to  the
master surface without applying any contact force. 
EQ.0:  logic is enabled (default), 
EQ.1:  logic 
is 
skipped 
for
(sometimes 
metalforming  calculations  or  for  contact  involving  foam
materials). 
recommended 
ISYM 
Symmetry plane option: 
EQ.0:  off, 
EQ.1:  do  not  include  faces  with  normal  boundary  constraints
(e.g., segments of brick elements on a symmetry plane). 
This option is important to retain the correct boundary conditions
in  the  model  with  symmetry.    For  the  ERODING  contacts  this
option may also be defined on card 4. 
I2D3D 
Segment searching option: 
EQ.0:  search  2D  elements  (shells)  before  3D  elements  (solids, 
thick shells) when locating segments. 
EQ.1:  search  3D  (solids,  thick  shells)  elements  before  2D
elements (shells) when locating segments.
VARIABLE   
SLDTHK 
SLDSTF 
DESCRIPTION
Optional  solid  element  thickness.    A  nonzero  positive  value  will
activate  the  contact  thickness  offsets  in  the  contact  algorithms
  The  contact  treatment  will  then  be
where  offsets  apply. 
equivalent to the case where null shell elements are used to cover
the  brick  elements.    The  contact  stiffness  parameter  below,
SLDSTF,  may  also  be  used  to  override  the  default  value.    This
parameter  applies  also  to  Mortar  contacts,  but  SLDSTF  is  then
ignored. 
Optional  solid  element  stiffness.    A  nonzero  positive  value
overrides  the  bulk  modulus  taken  from  the  material  model
referenced  by  the  solid  element.    For  segment  based  contact
(SOFT = 2),  SLDSTF  replaces  the  stiffness  used  in  the  penalty
equation.  This parameter does not apply to Mortar contacts.
*CONTACT_OPTION1_{OPTION2}_… 
Reminder:    If  Optional  Card  C  is  used,  then  Optional  Cards  A  and  B  must  be 
defined.  (Optional Cards A and B may be blank lines). 
Optional Card C. 
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IGAP 
IGNORE 
DPRFAC / 
MPAR1 
DTSTIF / 
MPAR2 
FLANGL  CID_RCF 
Type 
Default 
I 
1 
Remarks 
VARIABLE 
IGAP 
I 
0 
3 
F 
0 
1 
F 
0 
2 
F 
0 
I 
0 
DESCRIPTION 
For  mortar  contact  IGAP  is  used  to  progressively  increase  contact
stiffness  for  large  penetrations,  see  remarks  on  mortar  contact 
below. 
For  other  contacts  it  is  a  flag  to  improve  implicit  convergence
behavior at the expense of (1) creating some sticking if parts attempt
to  separate  and  (2)  possibly  underreporting  the  contact  force
magnitude  in  the  output  files  rcforc  and  ncforc.    (IMPLICIT 
ONLY.).  
LT.0:  Set  IGAP = 1  and  set  the  distance  for  turning  on  the
stiffness to  (IGAP/10) times the original distance.  
EQ.1:  Apply method to improve convergence (DEFAULT) 
EQ.2:  Do not apply method 
GT.2:  Set  IGAP = 1  for  first  IGAP − 2  converged  equilibrium 
states, then set IGAP = 2
VARIABLE 
IGNORE 
Ignore 
options. 
DESCRIPTION 
initial  penetrations 
in 
the  *CONTACT_AUTOMATIC 
LT.0:  Applies  only  to  the  Mortar  contact.    When  less  than  zero,
the  behavior  is  the  same  as  for  |IGNORE|,  but  contact  be-
tween segments belonging to the same part is ignored.  
The  main  purpose  of  this  option  is  to  avoid  spurious
contact  detections  that  otherwise  could  result  for  compli-
cated  geometries  in  a  single  surface  contact,  typically,
when  eliminating  initial  penetrations  by  interference.    See
IGNORE.EQ.3 and IGNORE.EQ.4. 
EQ.0:  Take  the  default  value  from  the  fourth  card  of  the  CON-
TROL_CONTACT input. 
EQ.1:  Allow  initial  penetrations  to  exist  by  tracking  the  initial
penetrations. 
EQ.2:  Allow  initial  penetrations  to  exist  by  tracking  the  initial
penetrations.  However, penetration warning messages are 
printed with the original coordinates and the recommend-
ed coordinates of each slave node given. 
EQ.3:  Applies only to the Mortar contact.  With this option initial
penetrations  are  eliminated  between  time  zero  and  the
time specified by MPAR1.  Intended for small initial pene-
trations.  See remarks on Mortar contact. 
EQ.4:  Applies only to the Mortar contact.  With this option initial
penetrations  are  eliminated  between  time  zero  and  the
time  specified  by  MPAR1.    In  addition  a  maximum  pene-
tration distance can be given as MPAR2, intended for large
initial penetrations.  See remarks on Mortar contact.
VARIABLE 
DPRFAC/ 
MPAR1 
DESCRIPTION 
Applies to the SOFT = 2 and Mortar contacts. 
Depth  of  penetration  reduction  factor  (DPRFAC)  for  SOFT = 2 
contact. 
EQ.0.0:  Initial penetrations are always ignored. 
GT.0.0:  Initial penetrations are penalized over time. 
LE.-1.0:  |DPRFAC|  is  the  load  curve  ID  defining  DPRFAC
versus time. 
For  the  mortar  contact  MPAR1  corresponds  to  initial  contact
pressure  in  interfaces  with  initial  penetrations  if  IGNORE = 2,  for 
IGNORE = 3,4  it  corresponds  to  the  time  of  closure  of  initial
penetrations.  See remarks below. 
DTSTIF/ 
MPAR2 
Applies to the SOFT = 1 and SOFT = 2 and Mortar contacts.  
Time  step  used  in  stiffness  calculation  for  SOFT = 1  and  SOFT = 2 
contact. 
EQ.0.0: 
Use  the  initial  value  that  is  used  for  time
integration. 
GT.0.0: 
Use the value specified. 
∈ (−1.0, −0.01): use  a  moving  average  of  the  solution  time  step.
(SOFT = 2 only) 
LE.-1.0: 
|DTSTIF|  is  the  ID  of  a  curve  that  defines 
DTSTIF vs.  time. 
For  the  mortar  contact  and  IGNORE = 4,  MPAR2  corresponds  a 
penetration depth that must be at least the penetration occurring in
the contact interface.  See remarks below. 
FLANGL 
Angle  tolerance  in  radians  for  feature  lines  option  in  smooth 
contact. 
EQ.0.0:  No feature line is considered for surface fitting in smooth
contact. 
GT.0.0:  Any  edge  with  angle  between  two  contact  segments
bigger than this angle will be treated as feature line dur-
ing surface fitting in smooth contact. 
CID_RCF 
Coordinate  system  ID  to  output  rcforc  force  resultants  and  ncforc
data in a local system.
Remarks: 
1.  DPRFAC/MPAR1  is  used  only  by  segment  based  contact  (SOFT = 2)  and 
Mortar Contact  .   By  default, 
SOFT = 2  contact  measures  the  initial  penetration  between  segment  pairs  that 
are found to be in contact and subtracts the measured value from the total pene-
tration for as long as a pair of segments remains in contact.  The penalty force is 
proportional  to  this  modified  value.    This  approach  prevents  shooting  nodes, 
but may allow unacceptable penetration.  DPRFAC can be used to decrease the 
measured value over time until the full penetration is penalized.  Setting DPR-
FAC = 0.01  will  cause  ~1%  reduction  in  the  measured  value  each  cycle.    The 
maximum allowable value for DPRFAC is 0.1.   A small value such as 0.001 is 
recommended.    DPRFAC  does  not  apply  to  initial  penetrations  at  the  start  of 
the calculation, only those that are measured at later times.  This prevents non-
physical movement and energy growth at the start of the calculation. 
2.  The anticipated use for the load curve option is to allow the initial penetrations 
to be reduced at the end of a calculation if the final geometry is to be used for a 
subsequent analysis.  To achieve this, load curve should have a y-value of zero 
until a time near the end of the analysis and then ramp up to a positive value 
such as 0.01 near the end of the analysis. 
3.  DTSTIF/MPAR2  is  used  only  by  the  SOFT = 1  and  SOFT = 2  contact  options 
and  the  Mortar  contact  (for  the  latter,  see remarks  on  Mortar  contact).    By  de-
fault  when  the  SOFT option  is  active,  the  contact  uses  the  initial  solution  time 
step to scale the contact stiffness.  If the user sets DTSTIF to a nonzero value, the 
inputted value will be used.  Because the square of the time step appears in the 
denominator of the stiffness calculation, a DTSTIF value larger than the initial 
solution time step reduces the contact stiffness and a smaller value increases the 
stiffness.  This option could be used when one component of a larger model has 
been analyzed independently and validated.  When the component is inserted 
into  the  larger  model,  the  larger  model  may  run  at  a  smaller  time  step  due  to 
higher mesh frequencies.  In the full model analysis, setting DTSTIF equal to the 
component analysis time step for the contact interface that treats the component 
will cause consistent contact stiffness between the analyses. 
The  load  curve  option  allows  contact  stiffness  to  be  a  function  of  time.    This 
should be done with care as energy will not be conserved.  A special case of the 
load  curve  option  is  when  |DTSTIF| = LCTM  on  *CONTROL_CONTACT.  
LCTM sets an upper bound on the solution time step.  For |DTSTIF| = LCTM, 
the contact stiffness time step value will track LCTM whenever the LCTM value 
is less than the initial solution time step.  If the LCTM value is greater, the initial 
solution time step is used.  This option could be used to stiffen the contact at the 
end  of  an  analysis.    To  achieve  this,  the  LCTM  curve  should  be  defined  such 
that  it  is  larger  than  the  solution  time  step  until  near  the  end  of  the  analysis.
Then the LCTM curve should ramp down below the solution time step causing 
it to decrease and the contact to stiffen.  A load curve value of 0.1 of the calcu-
lated  solution  time  step  will  cause  penetrations  to  reduce  by  about  99%.    To 
prevent  shooting  nodes,  the  rate  at  which  the  contact  stiffness  increases  is  au-
tomatically limited.  Therefore, to achieve 99% reduction, the solution should be 
run for perhaps 1000 cycles with a small time step. 
For segment based contact (SOFT = 2), setting DTSTIF less than or equal to -0.01 
and  greater  than  -1.0,  causes  the  contact  stiffness  to  be  updated  based  on  the 
current  solution  time  step.    Varying  the  contact  stiffness  during  a  simulation 
can  cause  energy  growth  so  this  option  should  be  used  with  care  when  extra 
stiffness  is  needed  to  prevent  penetration  and  the  solution  time  step  has 
dropped from the initial.  Because quick changes in contact stiffness can cause 
shooting  nodes,  using  a  moving  average of the  solution  time  step can  prevent 
this.  The value of DTSTIF determines the number of terms in the moving aver-
age  where  n = 100 ×  (-DTSTIF)  such  that  n = 1  for  DTSTIF = -0.01  and  n = 100 
for  DTSTIF = -0.999.    Setting  DTSTIF = -1.0  triggers  the  load  curve  option  de-
scribed in the previous paragraph, so DTSTIF cannot be smaller than -0.999 for 
this option. 
4.  When  SOFT = 2  on  Optional  Card  A  of  *CONTACT,  treatment  of  initial 
penetrations is always like IGNORE = 1 in that initial penetrations are ignored 
when calculating penalty forces.  If SOFT = 2 and IGNORE = 2, then a report of 
initial penetrations will be written to the messag file(s) in the first cycle.
Optional Card D: 
Reminder:  If Optional Card D is used, then Optional Cards A, B and C must be 
defined.  (Optional Cards A, B and C may be blank lines). 
Optional Card D. 
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Q2TRI 
DTPCHK 
SFNBR 
FNLSCL  DNLSCL 
TCSO 
TIEDID 
SHLEDG 
Type 
Default 
Remarks 
I 
0 
1 
  VARIABLE   
Q2TRI 
F 
0 
2 
F 
0 
3 
F 
0 
5 
F 
0 
5 
I 
0 
I 
0 
4 
I 
DESCRIPTION
Option  to  split  quadrilateral  contact  segments  into  two  triangles
(only available when SOFT = 2). 
EQ.0:  Off (default). 
EQ.1:  On for all slave shell segments. 
EQ.2:  On for all master shell segments. 
EQ.3:  On for all shell segments. 
EQ.4:  On for all shell segments of material type 34. 
DTPCHK 
Time interval between shell penetration reports (only available for
segment based contact) 
EQ.0.0:  Off (default). 
GT.0.0:  Check  and  report  segment  penetrations  at  time
intervals equal to DTPCHK
SFNBR 
*CONTACT_OPTION1_{OPTION2}_… 
DESCRIPTION
Scale  factor  for  neighbor  segment  contact  (only  available  for
segment based contact) 
EQ.0.0:  Off (default). 
GT.0.0:  Check neighbor segments for contact 
LT.0.0:  Neighbor  segment  checking  with  improved  energy
balance  when  |SFNBR| < 1000.    |SFNBR|≥1000  acti-
vates a split-pinball based neighbor contact with a pen-
alty force scale factor of |SFNBR+1000|.  For example, 
force scale factor used is 2 when SFNBR = -1002. 
FNLSCL 
Scale factor for nonlinear force scaling. 
TCSO 
Option  to  consider  only  contact  segments  (not  all  attached
elements)  when  computing  the  contact  thickness  for  a  node  or 
(for  SEGMENT_TO_SEGMENT  contact  and  shell 
segment 
elements only) 
EQ.0:  Off (default). 
EQ.1:  Only consider segments in the contact definition 
DNLSCL 
Distance for nonlinear force scaling. 
TIEDID 
Incremental displacement update for tied contacts.   
EQ.0:  Off (default). 
EQ.1:  On 
SHLEDG 
Flag  for  assuming  edge  shape  for  shells  when  measuring
penetration.  This is available for segment based contact  
EQ.0:  default to SHLEDG on *CONTROL_CONTACT 
EQ.1:  Shell  edges  are  assumed  square  and  are  flush  with  the
nodes 
EQ.2:  Shell  edges  are  assumed  round  with  radius  equal  to  ½
shell thickness
Remarks: 
1.  Q2TRI.  Setting Q2TRI to a nonzero value causes quadrilateral shell segments to 
be spilt into two triangles.  The contact segments only are split.  The elements 
are not changed.  This option is only available for segment based contact which 
is activated by setting SOFT = 2. 
2.  DTPCHK (Penetration Check).  Setting DTPCHK to a positive value causes a 
penetration check to be done periodically with the interval equal to DTPCHK.  
The check looks for shell segments that are penetrating the mid-plane of anoth-
er  shell  segment.    It  does  not  report  on  penetration  of  thickness  offsets.    The 
penetrating pairs are reported to the messag file or files for MPP.  If at least one 
penetration is found, the total number of pairs is reported to the screen output.  
This  option  is  only  available  for  segment  based  contact  which  is  activated  by 
setting SOFT = 2. 
3.  SFNBR.    SFNBR  is  a  scale  factor  for  optional  neighbor  segment  contact 
checking.    This  is  available  only  in  segment  based  (SOFT=2)  contact.    This  is 
helpful  option  when  a  mesh  folds  as  can  happen  with  compression  folding  of 
an airbag.  Only shell element segments are checked.  Setting SFNBR to a nega-
tive  value  modifies  the  neighbor  checking  to  improve  energy  balance.    When 
used, a value between -0.5 and -1.0 is recommended. 
4.  Round  off  in  OFFSET  and  TIEBREAK.    There  have  been  several  issues  with 
tied OFFSET contacts and AUTOMATIC_TIEBREAK contacts with offsets creat-
ing  numerical  round-off  noise  in  stationary parts.    By  computing  the  interface 
displacements  incrementally  rather  than  using  total  displacements,  the  round-
off  errors  that  occur  in  single  precision  are  eliminated.    The  incremental  ap-
proach is available for the following contact types: 
TIED_SURFACE_TO_SURFACE_OFFSET 
TIED_NODES_TO_SURFACE_OFFSET  
TIED_NODES_TO_SURFACE_CONSTRAINED_OFFSET 
TIED_SHELL_EDGE_TO_SURFACE_OFFSET 
AUTOMATIC_…_TIEBREAK  
5.  FNLSCL.    FNLSCL = 𝑓   and  DNLSCL = 𝑑  invoke  alternative  contact  stiffness 
scaling options.   
When FNLSCL > 0 and DNLSCL > 0, the first option scales the stiffness by the 
depth  of  penetration  to  provide  smoother  initial  contact  and  a  larger  contact 
force as the depth of penetration exceeds DNLSCL.  The stiffness k is scaled by 
the relation
𝑘 → 𝑘𝑓 √
where  𝛿  is  the  depth  of  penetration,  making  the  penalty  force  proportional  to 
the  3/2  power  of  the  penetration  depth.    Adding  a  small  amount  of  surface 
damping (e.g., VDC = 10) is advised with this option. 
When  SOFT = 2  and  FNLSCL < 0,  DNLSCL > 0,  an  alternative  stiffness  scaling 
scheme is used, 
𝑘 → 𝑘 [
0.01𝑓 𝐴𝑜
𝑑(𝑑 − 𝛿)
] 
where 𝐴0 is the overlap area of segments in contact.  For 𝛿 greater than 0.9𝑑, the 
stiffness is extrapolated to prevent it from going to infinity. 
When  SOFT = 2,  FNLSCL > 0,  and  DNLSCL = 0,  an  option  to  scale  the  contact 
by the overlap area is invoked. 
𝑘 → 𝑘𝑓 (
𝐴𝑜
𝐴𝑚
 ) 
where 𝐴𝑚 is the mean area of all the contact segments in the contact interface.  
This  third  option  can  improve  friction  behavior,  particularly  when  the  FS = 2 
option is used.
Optional Card E: 
Reminder:  If Optional Card E is used, then Optional Cards A, B, C and D must 
be defined.  (Optional Cards A, B, C and D may be blank lines). 
Optional Card E. 
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SHAREC  CPARM8 
IPBACK 
SRNDE 
FRICSF 
ICOR 
FTORQ 
REGION 
Type 
Default 
Remarks 
I 
0 
1 
I 
0 
I 
0 
2 
I 
0 
3 
F 
1. 
5 
I 
0 
I 
0 
I 
0 
4 
  VARIABLE   
DESCRIPTION
SHAREC 
Shared constraint flag (only available for segment based contact) 
CPARM8 
EQ.0:  Segments that share constraints not checked for contact.
EQ.1:  Segments that share constraints are checked for contact. 
This  variable  is  similar  to  CPARM8  in  *CONTACT_…_MPP  but 
applies to SMP and not to MPP.  CPARM8 for SMP only controls 
treatment  of  spot  weld  beams  in  CONTACT_AUTOMATIC_-
GENERAL.  
EQ.0:  Spot  weld  (type  9)  beams  are  not  considered  in  the 
contact even if included on the slave side of the contact. 
EQ.2:  Spot weld (type 9) beams are considered in the contact if
included on the slave side of the contact. 
IPBACK 
If set to a nonzero value, creates a “backup” penalty tied contact 
for this interface.  This option applies to constrained tied contacts
only.  See Remark 2.
SRNDE 
*CONTACT_OPTION1_{OPTION2}_… 
DESCRIPTION
Flag  for  non-extended  exterior  shell  edges.    See  Remark  3  below
for further information and restrictions:  
EQ.0:  Exterior shell edges have their usual treatment where the 
contact surface extends beyond the shell edge. 
EQ.1:  The contact surface is rounded at exterior shell edges but
does not extend beyond the shell edges.    
EQ.2:  The shell edges are square. 
FRICSF 
Scale factor for frictional stiffness (available for SOFT = 2 only). 
ICOR 
FTORQ 
If  set  to  a  nonzero  value,  VDC  is  the  coefficient  of  restitution
expressed  as  a  percentage.    When  SOFT = 0  or  1,  this  option 
applies  to  AUTOMATIC_NODES_TO_SURFACE,  AUTOMAT-
IC_SURFACE_TO_SURFACE  and  AUTOMATIC_SINGLE_SUR-
FACE.  When SOFT = 2, it applies to all available keywords. 
If  set  to  1,  a  torsional  force  is  computed  in  the  beam  to  beam
portion  of  contact 
type  AUTOMATIC_GENERAL,  which 
balances  the  torque  produced  due  to  friction.    This  is  currently 
only available in the MPP version. 
REGION 
The ID of a *DEFINE_REGION which will delimit the volume of 
space where this contact is active.  See Remark 4 below. 
Remarks: 
1.  The  SHAREC  flag  is  a  segment  based  contact  option  that  allows  contact 
checking  of  segment  pairs  that  share  a  multi-point  constraint  or  rigid  body.  
Sharing a constraint is defined as having at least one node of each segment that 
belongs to the same constraint. 
2.  The IPBACK flag is only applicable to constraint based tied contacts (TIED with 
no  options,  or  with  CONSTRAINED_OFFSET).    An  identical  penalty  based 
contact  is  generated  with  type  OFFSET,  except  in  the  case  of  SHELL_EDGE 
constrained  contact  which  generates  a  BEAM_OFFSET  type.    The  ID  of  the 
generated interface will be set to the ID of the original interface plus 1 if that ID 
is available, otherwise one more than the maximum used contact ID.  For nodes 
successfully tied by the constraint interface, the extra penalty tying should not 
cause  problems,  but  nodes  dropped  from  the  constraint  interface  due  to  rigid 
body or other conflicting constraints will be handled by the penalty contact.  In 
MPP, nodes successfully tied by the constraint interface are skipped during the 
penalty contact phase.
3.  The SRNDE option only applies to SOFT = 0 and SOFT = 1 contacts in the MPP 
version.   Shell  edges  for these  contacts  are  by  default  treated  by  adding  cylin-
drical caps along the free edges, with the radius of the cylinder equal to half the 
thickness of the  segment.  This has the side  effect of extending the segment at 
the  free  edges,  which  can  cause  problems.    Setting  SRNDE = 1  “rounds  over” 
the (through the thickness) corners of the element instead of extending it.  The 
edges of the segment are still rounded, but the overall size of the contact area is 
not  increased.    The  effect  is  as  if  the  free  edge  of  the  segment  was  moved  in 
toward the segment by a distance equal to half the segment thickness, and then 
the old cylindrical treatment was performed.  Setting SRNDE = 2 will treat the 
shell  edges  as  square,  with  no  extension.    This  variable  has  no  effect  on  shell-
edge-to-shell-edge interaction in AUTOMATIC_GENERAL; for that, see CPAR-
M8 on the MPP Card. 
The SRNDE = 1 option is available for the AUTOMATIC_SINGLE and AUTO-
MATIC_GENERAL contacts.  The NODE_TO_SURFACE and SURFACE_TO_-
SURFACE contacts also support SRNDE = 1 if the GROUPABLE option is used.   
The  SRNDE = 2  option  is  available  for  all  these  contact  types  if  the  GROUPA-
BLE option is enabled. 
4.  Setting a non-zero value for REGION does not limit or in any way alter the list 
of  slave  or  master  nodes  or  segments,  and  this  option  should  not  be  used  for 
that purpose.  For efficiency, the smallest possible portion of the model should 
be defined as slave or master using the normal mechanisms for specifying the 
slave  and  master  surfaces.    Setting  a  non-zero  value  will,  however,  result  in 
contact  outside  the  REGION  being  ignored.    As  slave  and  master  nodes  and 
segments pass into the indicated REGION, contact for them will become active.  
As they pass out of the REGION, they will be skipped in the contact calculation.  
This  option  is  currently  only  available  for  the  MPP  version,  and  only  for  con-
tacts  of  type  AUTOMATIC_SINGLE_SURFACE,  and  AUTOMATIC_*_TO_-
SURFACE. 
5.  The FRICSF factor is an optional factor to scale the frictional stiffness.  FRICSF 
is available only when SOFT = 2 on optional card A.  With penalty contact, the 
frictional  force  is  a  function  of  the  stiffness,  the  sliding  distance,  and  the  Cou-
lomb limit.
*CONTACT_OPTION1_{OPTION2}_… 
Reminder:    If  Optional  Card  F  is  used,  then  Optional  Cards  A,  B,  C,  D  and  E 
must be defined.  (Optional Cards A, B, C, D  and E may be blank lines). 
Optional Card F. 
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PSTIFF 
IGNROFF 
Type 
Default 
Remarks 
I 
0 
1 
  VARIABLE   
PSTIFF 
I 
 0 
DESCRIPTION
Flag  to  choose  the  method  for  calculating  the  penalty  stiffness.
This is available for segment based contact  
EQ.0:  Use  the  default  as  defined  by  PSTIFF  on  *CONTROL_-
CONTACT. 
EQ.1:  Based on nodal masses 
EQ.2:  Based on material density and segment dimensions. 
IGNROFF 
Flag  to  ignore  the  thickness  offset  for  shells  in  the  calculation  of
the shell contact penetration depth.  This allows shells to be used
for  meshing  rigid  body  dies  without  modifying  the  positions  of 
the nodes to compensate for the shell thickness. 
EQ.1:  Ignore the master side thickness. 
EQ.2:  Ignore the slave side thickness. 
EQ.3:  Ignore the thickness of both sides..
Remarks: 
1.  See  Remark  6  on  *CONTROL_CONTACT  for  an  explanation  of  the  PSTIFF 
option.    Specifying  PSTIFF  here  will  override  the  default  value  as  defined  by 
PSTIFF on *CONTROL_CONTACT. 
General Remarks: *CONTACT 
1.  Modeling  airbag  interactions  with  structures  and  occupants  using  the  actual 
fabric thickness, which is approximate 0.30 mm, may result in a contact break-
down that leads to inconsistent occupant behavior between different machines.  
Based  on  our  experience,  using  a  two-way  automatic  type  contact  definition, 
i.e.,  AUTOMATIC_SURFACE_TO_SURFACE,  between  any  airbag  to  struc-
ture/occupant  interaction  and  setting  the  airbag  fabric  contact  thickness  to  at 
least 10 times the actual fabric thickness has helped improved contact behavior 
and eliminates the machine inconsistencies.  Due to a large stiffness difference 
between  the  airbag  and  the  interacting  materials,  the  soft  constraint  option 
(SOFT = 1) or the segment based option (SOFT = 2) is recommended.  It must be 
noted  that  with  the  above  contact  definition,  only  the  airbag  materials  should 
be included in any *AIRBAG_SINGLE_SURFACE definitions to avoid duplicate 
contact treatment that can lead to numerical instabilities. 
2.  The following contact definitions are based on constraint equations and will not 
work with rigid bodies: 
TIED_NODES_TO_SURFACE  
TIED_NODES_TO_SURFACE_CONSTRAINED_OFFSET  
TIED_SURFACE_TO_SURFACE 
TIED_SURFACE_TO_SURFACE_CONSTRAINED_OFFSET 
TIED_SHELL_EDGE_TO_SURFACE  
TIED_SHELL_EDGE_TO_SURFACE_CONSTRAINED_OFFSET  
TIED_SHELL_EDGE_TO_SOLID 
SPOTWELD 
SPOTWELD_WITH_TORSION 
However,  SPOTWELD_WITH_TORSION_PENALTY  does  work  with  rigid 
bodies and tied interfaces with the offset option can be used with rigid bodies, 
i.e.,
TIED_NODES_TO_SURFACE_OFFSET 
TIED_SHELL_EDGE_TO_SURFACE_OFFSET 
TIED_SHELL_EDGE_TO_SURFACE_BEAM_OFFSET 
TIED_SURFACE_TO_SURFACE_OFFSET 
Also, it may sometimes be advantageous to use the CONSTRAINED_EXTRA_-
NODE_OPTION instead for tying deformable nodes to rigid bodies since in this 
latter  case  the  tied  nodes  may  be  an  arbitrary  distance  away  from  the  rigid 
body. 
Tying  will  only  work  if  the  surfaces  are  near  each  other.    The  criteria  used  to 
determine  whether  a  slave  node  is  tied  down  is  that  it  must  be  “close”.    For 
shell elements “close” is defined as distance, 𝛿, less than: 
𝛿1 = 0.60 × (thickness of slave node + thickness of master segment) 
𝛿2 = 0.05 × min(master segment diagonals) 
𝛿 = max(𝛿1, 𝛿2) 
If  a  node  is  further  away  it  will  not  be  tied  and  a  warning  message  will  be 
printed.    For  solid  elements  the  slave  node  thickness  is  zero  and  the  segment 
thickness  is  the  element  volume  divided  by  the  segment  area;  otherwise,  the 
same procedure is used. 
If there is a large difference in element areas between the master and slave side, 
the distance,  𝛿2, may be too large and may cause the unexpected projection of 
nodes that should not be tied.  This can occur during calculation when adaptive 
remeshing is used.  To avoid this difficulty the slave and master thickness can 
be specified as negative values on Card 3 in which case  
𝛿 = abs(𝛿1) 
3.  The contact algorithm for tying spot welds with torsion, SPOTWELD_WITH_-
TORSION, must be used with care.  Parts that are tied by this option should be 
subjected  to  stiffness  proportional  damping  of  approximately  ten  percent,  i.e., 
input  a  coefficient  of  0.10.    This  can  be  defined  for  each  part  on  the  *DAMP-
ING_PART_STIFFNESS input.  Stability problems may arise with this option if 
damping  is  not  used.    This  comment  applies  also  to  the  PENALTY  keyword 
option. 
4.  These  contact  definitions  must  be  used  with  care.    The  surface  and  the  nodes 
which  are  constrained  to  a  surface  are  not  allowed  to  be  used  in  any  other 
CONSTRAINT_… contact definition: 
CONSTRAINT_NODES_TO_SURFACE
CONSTRAINT_SURFACE_TO_SURFACE 
If, however, contact has to be defined from both sides as in sheet metal forming, 
one  of  these  contact  definitions  can  be  a  CONSTRAINT  type;  the  other  one 
could  be  a  standard  penalty  type  such  as  SURFACE_TO_SURFACE  or 
NODES_TO_SURFACE. 
5.  These  contact  definitions  require  thickness  to  be  taken  into  account  for  rigid 
bodies modeled with shell elements.  Therefore, care should be taken to ensure 
that realistic thicknesses are specified for the rigid body shells. 
AIRBAG_SINGLE_SURFACE 
AUTOMATIC_GENERAL 
AUTOMATIC_GENERAL_INTERIOR 
AUTOMATIC_NODES_TO_SURFACE 
AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE 
AUTOMATIC_SINGLE_SURFACE  
AUTOMATIC_SURFACE_TO_SURFACE 
SINGLE_SURFACE 
A thickness that is too small may result in loss of contact and an unrealistically 
large thickness may result in a degradation in speed during the bucket sorts as 
well  as  nonphysical  behavior.    The  SHLTHK  option  on  the  *CONTROL_CON-
TACT card is ignored for these contact types. 
6.  Two  methods  are  used  in  LS-DYNA  for  projecting  the  contact  surface  to 
account for shell thicknesses.  The choice of methods can influence the accuracy 
and cost of the calculation.  Segment based projection is used in contact types:  
 
AIRBAG_SINGLE_SURFACE  
AUTOMATIC_GENERAL 
AUTOMATIC_NODES_TO_SURFACE 
AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE 
AUTOMATIC_SINGLE_SURFACE  
AUTOMATIC_SURFACE_TO_SURFACE
Nodal normal projection 
Segment based projection
Figure  11-13.    Nodal  normal  and  segment  based  projection  is  used  in  the
contact options  
FORMING_NODES_TO_SURFACE 
FORMING_ONE_WAY_SURFACE_TO_SURFACE 
FORMING_SURFACE_TO_SURFACE 
The  remaining  contact  types  use  nodal  normal  projections  if  projections  are 
used.    The  main  advantage  of  nodal  projections  is  that  a  continuous  contact 
surface is obtained which is much more accurate in applications such as metal 
forming.  The disadvantages of nodal projections are the higher costs due to the 
nodal  normal  calculations,  difficulties  in  treating  T-intersections  and  other 
geometric  complications,  and  the  need  for  consistent  orientation  of  contact 
surface segments.  The contact type 
SINGLE_SURFACE 
uses nodal normal projections and consequently is slower than the alternatives. 
7.  These contact algorithms allow the total contact forces applied by all contacts to 
be picked up. 
FORCE_TRANSDUCER_PENALTY 
FORCE_TRANSDUCER_CONSTRAINT 
8.  This  contact  does  not apply  any  force  to the  model  and  will  have no  effect  on 
the solution.  Only the slave set and slave set type need be defined for this con-
tact type.  Generally, only the first three cards are defined.  The force transducer 
option, PENALTY, works with penalty type contact algorithms only, i.e., it does
Contact surface augment SLDTHK 
Contact surface augment (SST × SFST-T)/2
Element thickness T 
Figure  11-14.    Illustration  of  contact  surface  location  for  automatic  Mortar
contact, solids on top and shells below. 
not work with the CONSTRAINT or TIED options.  For these latter options, use 
the  CONSTRAINT  option.    If  a  transducer  is  used  for  extracting  forces  from 
Mortar  contacts,  the  slave  and  master  sides  must  be  defined  through  parts  or 
part sets, segment or node sets will not gather the correct data. 
NOTE: If  the  interactions  between  two  surfaces  are  needed, 
a master surface should be defined.  In this case, only 
the  contact  forces  applied  between  the  slave  and 
master surfaces are kept.  The master surface option 
is  only  implemented  for  the  PENALTY  option  and 
works only with the AUTOMATIC contact types. 
9.  FORMING_…  These  contacts  are  mainly  used  for  metal  forming  applications.  
A connected mesh is not required for the master (tooling) side but the orienta-
tion of the mesh must be in the same direction.  These contact types are based 
on the AUTOMATIC type contacts and consequently the performance is better 
than the original two surface contacts. 
10.  The  mortar  contact,  invoked  by  appending  the  suffix  MORTAR  to  either 
FORMING_SURFACE_TO_SURFACE, 
AUTOMATIC_SURFACE_TO_SUR-
FACE  or  AUTOMATIC_SINGLE_SURFACE  is  a  segment  to  segment  penalty 
based contact.  For two segments on each side of the contact interface that are 
overlapping  and  penetrating,  a  consistent  nodal  force  assembly  taking  into 
account the individual shape functions of the segments is performed, see Figure 
11-16 for an illustration.  A TRANSDUCER_PENALTY can be used for extract-
ing forces from Mortar contacts, but the slave and master sides must then be defined 
through parts or part sets. 
In  this  respect  the  results  with  this  contact  may  be  more  accurate,  especially 
when  considering  contact  with  elements  of  higher  order.    By  appending  the 
suffix TIED to the CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_MOR-
TAR  keyword  or  the  suffix  TIEBREAK_MORTAR  (only  OPTION = 7  and  OP-
TION = 9  supported)  to  the  CONTACT_AUTOMATIC_SURFACE_TO_SUR-
FACE keyword, this is treated as a tied contact interface with optional failure in 
the latter case.  This contact is intended for implicit analysis in particular but is 
nevertheless  supported  for  explicit  analysis  as  well.    For  explicit  analysis,  the 
bucket sort frequency is 100 if not specified. 
The  FORMING  mortar  contact,  in  contrast  to  other  forming  contacts,  does  not 
assume a rigid master side, but if this side consists of shell elements the normal 
should  be  oriented  towards  the  slave  side.    Furthermore,  no  shell  thickness  is 
taken  into  account  on  the  master  side.    The  slave  side  is  assumed  to  be  a  de-
formable shell part, and the orientation of the elements does not matter.  How-
ever, each FORMING contact definition should be such that contact occurs with 
ONE  deformable  slave  side  only,  which  obviously  leads  to  multiple  contact 
definitions  if  two-sided  contact  is  presumed.    The  AUTOMATIC  contact  is 
supported for solids, shells and beams, and here the thicknesses are taken into 
account both for rigid and deformable parts.  Flat edge contact is supported for 
shell elements and contact with beams occurs on the lateral surface area as well 
as  on  the  end  tip.    The  contact  assumes  that  the  beam  has  a  cylindrical  shape 
with a cross sectional area coinciding with that of the underlying beam element.  
For  the  AUTOMATIC  contact,  the  contact  surface  can  be  augmented  with  the 
aid  of  parameters  SST  and  SFST  for  shells  and  beams,  while  SLDTHK  is  used 
for  solids  and  thick  shells.    For  shells/beams  SST  corresponds  to  the  contact 
thickness  of  the  element  (MST  likewise  for  the  master  side),  by  default  this  is 
the  same  as  the  element  thickness.    This  parameter  can  be  scaled  with  aid  of 
SFST (SFMT for the master side) to adjust the location of the contact surface, see 
Figure 11-14.  
For  solids  PENMAX  can  be  used  to  determine  the  maximum  penetration  and 
also determines the search depth for finding contact pairs, if set it should corre-
spond to a characteristic thickness in the model.  Also, the contact  surface can 
be  adjusted  with  the  aid  of  SLDTHK  if  it  is  of  importance  to  reduce  the  gap 
between parts, see Figure 11-14.  This may be of interest if initial gaps result in 
free objects undergoing rigid body motion and thus preventing convergence in 
implicit.
4
 3.5
 3
 2.5
 2
 1.5
 1
 0.5
 0
 0
IGAP=1 
IGAP=2 
IGAP=5 
IGAP=10
 0.2
 0.4
 0.6
 0.8
 1
Penetration
Figure 11-15.  Mortar contact stress as function of penetration 
For  the  TIED  option,  the  criterion  for  tying  two  contact  surfaces  is  by  default 
that the distance should be less than 0.05 × T, i.e., by default it is within 5% of 
the element thickness (characteristic size for solids).  In this case PENMAX can 
be used to set the tying distance, i.e., if PENMAX is positive then segments are 
tied if the distance is less than PENMAX. 
If initial penetrations are detected (reported in the messag file) then by default 
these  will  yield  an  initial  contact  stress  corresponding  to  this  level  of  penetra-
tion.    IGNORE > 0  can  be  used  to  prevent  unwanted  effects  of  this.    IG-
NORE = 2  behaves  differently  than  from  other  contacts,  for  this  option  the 
penetrations are not tracked but the contact surface is fixed at its initial location.  
In addition, for IGNORE = 2, an initial contact pressure can be imposed on the 
interface by setting the MPAR1 parameter to the desired contact pressure.  All 
this  allows  to  properly  eliminate  any  rigid  body  motion  due  to  initial  contact 
gaps.
4 
Slave 
1 
x3 
x2 
O 
x1 
Master segment 
Figure 11-16.  Illustration of Mortar segment to segment contact 
A third option is IGNORE = 3, for which prestress can be applied.  This allows 
initial penetrations to exists and they are closed during the time between zero 
and the value given by MPAR1, thus working pretty similar to the INTERFER-
ENCE option with the exception that the closure is linear in time.  A limitation 
with  IGNORE = 3  in  this  context  is  that  the  initial  penetrations  must  be  small 
enough for the contact algorithm to detect them.  
Thus,  for  large  penetrations  IGNORE = 4  is  recommended  (this  can  only  be 
used  if  the  slave  side  consists  of  solid  elements).    This  does  pretty  much  the 
same  thing  as  IGNORE = 3,  but  the  user  may  provide  a  penetration  depth  in 
MPAR2.  This depth must be at least as large as (and preferably in the order of) 
the  maximum  initial  penetration  in  the  contact  interface  or  otherwise  an  error 
termination will be the result.  The need for such a parameter is for the contact 
algorithm  to  have  a  decent  chance  to  locate  the  contact  surface  and  thus  esti-
mate  the  initial  penetration.    With  this  option  the  contact  surfaces  are  pushed 
back  and  placed  in  incident  contact  at  places  where  initial  penetrations  are 
present, this can be done for (more or less) arbitrary initial penetration depths.  
As  for  IGNORE = 3,  the  contact  surfaces  will  be  restored  linearly  in  the  time 
given by MPAR1.  
A problem with mortar contacts in implicit analysis could be that contact pres-
sure is locally very high and leads to large enough penetrations to be released 
in  subsequent  steps.    Penetration  information  can  be  requested  on  MINFO  on 
*CONTROL_OUTPUT  which  issues  a  warning  if  there  is  a  danger  for  this  to 
happen.  To prevent contact release the user may increase IGAP which penaliz-
es large penetrations without affecting small penetration behavior and thereby 
overall implicit performance. Figure 11-15  shows the contact pressure as func-
tion  of  penetration  for  the  mortar  contact,  including  the  effect  of  increasing 
IGAP.    It  also  shows  that  for  sufficiently  large  penetrations  the  contact  is  not 
detected in subsequent steps which is something to avoid.
INTERFACE 
TYPE ID 
PENCHK 
ELEMENT
TYPE 
FORMULA FOR RELEASE 
OF PENETRATING NODAL POINT 
0 
1 
2 
1, 2, 6, 7 
3, 5, 8, 9, 10 
(without thickness) 
3, 5, 10 (thickness), 17 
and 18 
a3, a5, a10, 13, 15 
4 
26 
solid 
shell 
solid 
shell 
solid 
shell 
solid 
shell 
solid 
d  =  PENMAX if PENMAX > 0 
d  =  1.e+10 if PENMAX = 0 
d  =  PENMAX if PENMAX > 0 
d  =  1.e+10 if PENMAX = 0 
d  =  XPENE × thickness of solid element 
d  =  XPENE thickness of shell element 
d  =  0.05 × minimum diagonal length 
d  =  0.05 × minimum diagonal length 
d  =  XPENE × thickness of solid element 
d  =  XPENE × thickness of shell element 
d  =  PENMAX × thickness of solid element 
[default: PENMAX = 0.5] 
d  =  PENMAX × (slave thickness + master 
shell 
thickness) 
[default: PENMAX = 0.4] 
solid 
d  =  0.5 × thickness of solid element 
shell 
solid 
d  =  0.4 ×  (slave thickness + master 
thickness) 
d  =  PENMAX × thickness of solid element 
[default: PENMAX = 10.0] 
d  =  PENMAX × (slave thickness + master 
shell 
thickness) 
 [default: PENMAX = 10.] 
Table  11-17.    Criterion  for  node  release  for  nodal  points  which  have 
penetrated  too  far.    This  criterion  does  not  apply  to  SOFT = 2  contact.  
Larger  penalty  stiffnesses  are  recommended  for  the  contact  interface 
which  allows  nodes  to  be  released.    For  node-to-surface  type  contacts  (5, 
5a) the element thicknesses which contain the node determines the nodal 
thickness.    The  parameter  is  defined  on  the  *CONTROL_CONTACT 
input.
Mapping of *CONTACT keyword option to “contact type” in d3hsp: 
Structured 
Input Type ID 
a 13 
  26 
i  26 
a 5 
a 5 
a  10 
  13 
a  3 
a  3 
  18 
  17 
  23 
  16 
  14 
  15 
  27 
  25 
m  5 
m  10 
m  3 
  5 
  5 
  10 
  20 
Keyword Name 
AIRBAG_SINGLE_SURFACE  
AUTOMATIC_GENERAL 
AUTOMATIC_GENERAL_INTERIOR 
AUTOMATIC_NODES_TO_SURFACE 
AUTOMATIC_NODES_TO_SURFACE_TIEBREAK 
AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE 
AUTOMATIC_SINGLE_SURFACE  
AUTOMATIC_SURFACE_TO_SURFACE 
AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK 
CONSTRAINT_NODES_TO_SURFACE 
CONSTRAINT_SURFACE_TO_SURFACE 
DRAWBEAD 
ERODING_NODES_TO_SURFACE 
ERODING_SURFACE_TO_SURFACE 
ERODING_SINGLE_SURFACE 
FORCE_TRANSDUCER_CONSTRAINT 
FORCE_TRANSDUCER_PENALTY 
FORMING_NODES_TO_SURFACE 
FORMING_ONE_WAY_SURFACE_TO_SURFACE 
FORMING_SURFACE_TO_SURFACE 
NODES_TO_SURFACE 
NODES_TO_SURFACE_INTERFERENCE 
ONE_WAY_SURFACE_TO_SURFACE 
RIGID_NODES_TO_RIGID_BODY
Structured 
Input Type ID 
  21 
  19 
  22 
  4 
  1 
Keyword Name 
RIGID_BODY_ONE_WAY_TO_RIGID_BODY 
RIGID_BODY_TWO_WAY_TO_RIGID_BODY 
SINGLE_EDGE 
SINGLE_SURFACE 
SLIDING_ONLY 
p  1 
SLIDING_ONLY_PENALTY 
  3 
  3 
  8 
  9 
  6 
o  6 
c  6 
  7 
o  7 
c  7 
b  7 
s  7 
  2 
o  2 
c  2 
SURFACE_TO_SURFACE 
SURFACE_TO_SURFACE_INTERFERENCE 
TIEBREAK_NODES_TO_SURFACE 
TIEBREAK_SURFACE_TO_SURFACE 
TIED_NODES_TO_SURFACE 
TIED_NODES_TO_SURFACE_OFFSET 
TIED_NODES_TO_SURFACE_CONSTRAINED_OFFSET 
TIED_SHELL_EDGE_TO_SURFACE or SPOTWELD 
TIED_SHELL_EDGE_TO_SURFACE_OFFSET 
TIED_SHELL_EDGE_TO_SURFACE_CONSTRAINED_OFFSET 
or SPOTWELD_CONSTRAINED_OFFSET 
TIED_SHELL_EDGE_TO_SURFACE_BEAM_OFFSET 
SPOTWELD_BEAM_OFFSET 
or 
SPOTWELD_WITH_TORSION 
TIED_SURFACE_TO_SURFACE 
TIED_SURFACE_TO_SURFACE_OFFSET 
TIED_SURFACE_TO_SURFACE_CONSTRAINED_OFFSET
*CONTACT_OPTION1_{OPTION2}_… 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *CONTACT_NODES_TO_SURFACE 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Make a simple contact that prevents the nodes in part 2 from 
$  penetrating the segments in part 3. 
$ 
*CONTACT_NODES_TO_SURFACE 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$     ssid      msid     sstyp     mstyp    sboxid    mboxid       spr       mpr 
         2         3         3         3 
$ 
$       fs        fd        dc        vc       vdc    penchk        bt        dt 
$ 
$      sfs       sfm       sst       mst      sfst      sfmt       fsf       vsf 
$ 
$    sstype, mstype = 3  id's specified in ssid and msid are parts 
$      ssid = 2  use slave nodes in part 2 
$      msid = 3  use master segments in part 3 
$ 
$  Use defaults for all parameters. 
$ 
$$$$  Optional Cards A and B not specified (default values will be used). 
$ 
$ 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *CONTACT_SINGLE_SURFACE 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Create a single surface contact between four parts: 28, 97, 88 and 92 
$     - create a part set with set ID = 5, list the four parts 
$     - in the *CONTACT_SINGLE_SURFACE definition specify: 
$           sstyp = 2  which means the value for ssid is a part set 
$           ssid  = 5  use part set 5 for defining the contact surfaces 
$ 
$  Additional contact specifications described below. 
$ 
*CONTACT_SINGLE_SURFACE 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$     ssid      msid     sstyp     mstyp    sboxid    mboxid       spr       mpr 
         5                   2 
$       fs        fd        dc        vc       vdc    penchk        bt        dt 
      0.08      0.05        10                  20                          40.0 
$      sfs       sfm       sst       mst      sfst      sfmt       fsf       vsf 
$ 
$       fs = 0.08  static coefficient of friction equals 0.08 
$       fd = 0.05  dynamic coefficient of friction equals 0.05 
$       dc =   10  exponential decay coefficient, helps specify the transition 
$                     from a static slide to a very dynamic slide 
$      vdc =   20  viscous damping of 20% critical (damps out nodal
$                     oscillations due to the contact) 
$       dt = 40.0  contact will deactivate at 40 ms (assuming time unit is ms) 
$ 
$$$$  Optional Cards A and B not specified (default values will be used). 
$ 
$ 
*SET_PART_LIST 
$      sid 
         5 
$     pid1      pid2      pid3      pid4 
        28        97        88        92 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *CONTACT_DRAWBEAD 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Define a draw bead contact: 
$    - the draw bead is to be made from the nodes specified in node set 2 
$    - the master segments are to be those found in the box defined by box 2 
$        that are in part 18 
$    - include slave and master forces in interface file (spr, mpr = 1) 
$ 
*CONTACT_DRAWBEAD 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$     ssid      msid     sstyp     mstyp    sboxid    mboxid       spr       mpr 
         2        18         4         3                   2         1         1 
$ 
$       fs        fd        dc        vc       vdc    penchk        bt        dt 
      0.10           
$ 
$      sfs       sfm       sst       mst      sfst      sfmt       fsf       vsf 
$ 
$$$$ Card 4 required because it's a drawbead contact 
$ 
$  lcdidrf    lcidnf     dbdth     dfscl    numint 
         3             0.17436       2.0 
$ 
$  lcdidrf =       3  load curve 3 specifies the bending component of the 
$                       restraining force per unit draw bead length 
$    dbdth = 0.17436  draw bead depth 
$    dfscl =     2.0  scale load curve 3 (lcdidrf) by 2 
$ 
$$$$  Optional Cards A and B not specified (default values will be used). 
$ 
*DEFINE_BOX 
$    boxid       xmm       xmx       ymn       ymx       zmn       zmx 
         2 0.000E+00 6.000E+00 6.000E+00 1.000E+02-1.000E+03 1.000E+03 
$ 
*SET_NODE_LIST 
$      sid       da1       da2       da3       da4 
         2 
$     nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
      2580      2581      2582      2583      2584      2585      2586      2587 
      2588      2589      2590 
$ 
*DEFINE_CURVE 
$     lcid      sidr      scla      sclo      offa      offo 
         3 
$                  a                   o 
$              DEPTH           FORC/LGTH
0.000E+00           0.000E+00 
           1.200E-01           1.300E+02 
           1.500E-01           2.000E+02 
           1.800E-01           5.000E+02
*CONTACT 
This  card  associates  a  wear  model  to  a  contact  interface  for  post-processing  wear 
quantities. 
This card does not affect the results of a simulation.  Wear is associated to friction so the 
frictional  coefficient  must  be  nonzero  for  the  associated  contact  interface.    This  feature 
calculates  the  wear  depth,  sliding  distance  and  possibly  user  defined  wear  history 
variables according to the specified model and writes it to the intfor database for post-
processing.    Note  that  this  data  is  not  written  unless  the  parameter  NWEAR  and/or 
NWUSR are set on the *DATABASE_EXTENT_INTFOR card.  𝐻-adaptive remeshing is 
supported  with  this  feature.    Implicit  analysis  is  supported,  for  which  mortar  is  the 
preferred contact. 
  Card 1 
1 
2 
Variable 
CID 
WTYPE 
Type 
I 
I 
3 
P1 
F 
4 
P2 
F 
5 
P3 
F 
6 
P4 
F 
7 
P5 
F 
8 
P6 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
User Defined Wear Parameter Cards.  Define as many cards as needed to define P1 
parameters if and only if WTYPE.LT.0.  
  Card n 
1 
Variable 
W1 
2 
W2 
3 
W3 
4 
W4 
5 
W5 
6 
W6 
7 
W7 
8 
W8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
CID 
Contact interface ID, see *CONTACT_…
VARIABLE   
DESCRIPTION
WTYPE 
Wear law 
LT.0:  User  defined  wear  law,  value  specifies  type  used  in 
subroutine. 
EQ.0: Archard’s wear law. 
P1 
First wear parameter 
WTYPE.EQ.0: Dimensionless  scale  factor  𝑘.    If  negative  the 
ID  with
absolute  value  specifies  a 
𝑘 = 𝑘(𝑝, 𝑑 ̇) as a function of contact pressure 𝑝 ≥ 0
and relative sliding velocity 𝑑 ̇≥ 0. 
table 
WTYPE.LT.0:  Number  of  user  wear  parameters  for  this
interface. 
P2 
Second wear parameter 
WTYPE.EQ.0: Slave surface hardness parameter 𝐻𝑠.  If negative 
the  absolute  value  specifies  a  curve  ID  with
𝐻𝑠 = 𝐻𝑠(𝑇𝑠)  as  function  of  slave  node  tempera-
ture 𝑇𝑠. 
WTYPE.LT.0:  Number  of  user  wear  history  variables  per
contact  node,  these  can  be  output  to  the  intfor
file,  see  NWUSR  on  *DATABASE_EXTENT_-
INTFOR. 
P3 
Third wear parameter 
WTYPE.EQ.0: Master  surface  hardness  parameter  𝐻𝑚. 
  If 
negative  the  absolute  value  specifies  a  curve  ID
with   𝐻𝑚 = 𝐻𝑚(𝑇𝑚)  as  function  of  master  node 
temperature 𝑇𝑚. 
WTYPE.LT.0:  Not used. 
P4 - P6 
Not used. 
WN 
Nth user defined wear parameter. 
Remarks: 
Archard’s  wear  law  (WTYPE.EQ.0)  states  that  the  wear  depth  𝑤  at  a  contact  point 
evolves with time as
𝑤̇ = 𝑘
𝑝𝑑 ̇
where 𝑘 > 0 is a dimensionless scale factor, 𝑝 ≥ 0 is the contact interface pressure, 𝑑 ̇≥ 0 
is the relative sliding velocity of the points in contact and 𝐻 > 0 is the surface hardness 
(force  per  area).    The  wear  depth  for  a  node  in  contact  is  incremented  in  accordance 
with  this  formula,  accounting  for  different  hardness  of  the  slave  and  master  side,  𝐻𝑠 
and 𝐻𝑚, respectively.  By using negative numbers for wear parameters P1, P2 or P3, the 
corresponding parameter is defined by a table or a curve.  For P1, the value of 𝑘 is taken 
from a table with contact pressure 𝑝 and sliding velocity 𝑑 ̇ as arguments, while for P2 or 
P3,  the  corresponding  hardness  𝐻  is  taken  from  curves  with  the  associated  contact 
nodal temperature 𝑇 as argument.  That is, the slave side hardness will be a function of 
the slave side temperature, and vice versa. 
Customized wear laws may be specified as a user-defined subroutine called userwear.  
This subroutine is called when WTYPE < 0.  This subroutine is passed wear parameters 
  for  this  interface  as  well  as  number  of  wear  history  variables    per 
contact node.  The wear parameters are defined on additional cards  and the 
history  variables  are  updated  in  the  user  subroutine.    The  history  variables  can  be 
output to the intfor file, see NWUSR on *DATABASE_EXTENT_INTFOR.  WTYPE may 
be  used  to  distinguish  between  different  wear  laws,  and  consequently  any  number  of 
different laws can be implemented within the same subroutine.  For more information, 
we  refer  to  the  source  code  which  contains  extensive  commentaries  and  two  sample 
wear laws. 
Only one wear law per contact interface can be specified.  The procedure for activating 
this feature involves 
1.  Using the present keyword to associate wear to a contact interface 
2.  Setting NWEAR and/or NWUSR on the *DATABASE_EXTENT_INTFOR card. 
3.  Having a contact interface with friction of a type that is supported..  If SOFT = 2 
on  optional  card A  of the  contact  data, then any  valid keyword option  is  sup-
ported.  If SOFT = 0 or SOFT = 1, then the following list is supported. 
*CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE 
*CONTACT_FORMING_SURFACE_TO_SURFACE 
*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE 
*CONTACT_FORMING_SURFACE_TO_SURFACE_MORTAR 
*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_MORTAR 
*CONTACT_AUTOMATIC_SINGLE_SURFACE_MORTAR
1. 
_SMOOTH option is not supported 
2.  MPP “groupable” option is not supported 
*CONTACT_ADD_WEAR 
See  also  *DATABASE_EXTENT_INTFOR  for  general  guidelines  related  to  the  intfor 
database.
*CONTACT 
Purpose:    This  feature  allows  for  automatic  move  of  a  master  surface  in  a  contact 
definition to close an unspecified gap between a slave and the master surface.  The gap 
may be caused as a result of an initial gravity loading on the slave part.  The gap will be 
closed  on  a  specified  time  to  save  CPU  time.    The  master  surface  in  metal  forming 
application will typically be the upper cavity and the slave part will be the blank.  This 
feature is applicable only for sheet metal forming application. 
  Cards 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
CONTID 
VID 
LCID 
ATIME 
OFFSET 
Type 
I 
I 
I 
Default 
none 
none 
none 
I 
0 
F 
F 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
ID 
Move ID for this automatic move input. 
CONTID 
VID 
LCID 
GT.0: velocity  controlled  tool  kinematics  (the  variable  VAD = 0 
in *BOUNDARY_PRESCRIBED_MOTION_RIGID) 
LT.0:  displacement controlled tool kinematics (VAD = 2) 
Contact  ID,  as  in  *CONTACT_FORMING_...._ID,  which  defines 
the slave and master part set IDs. 
Vector ID of a vector oriented in the direction of movement of the 
master surface, as in *DEFINE_VECTOR.  The origin of the vector 
is  unimportant  since  the  direction  cosines  of  the  vector  are
computed and used. 
Load  curve  defining  tooling  kinematics,  either  by  velocity  versus
time  or  by  displacement  versus  time.    This  load  curve  will  be
adjusted automatically during a simulation to close the empty tool
travel. 
ATIME 
Activation  time  defining  the  moment  the  master  surface  (tool)  to 
be moved.
OFFSET 
*CONTACT_AUTO_MOVE 
DESCRIPTION
Time at which a master surface will move to close a gap distance,
which may happen following the move of another master surface.
This  is  useful  in  sequential  multiple  flanging  or  press  hemming
simulation.    Simulation  time  (CPU)  is  much  faster  based  on  the 
shortened tool travel (no change to the termination time). 
Example: gravity loading and closing with implicit static 
Referring  to  the  partial  input  deck  below  and  Figure  11-18,  a  combined  simulation  of 
gravity  loading  and  binder  closing  of  a  fender  outer  is  demonstrated  on  the 
NUMISHEET  2002  benchmark.    In  this  multi-step  implicit  static  set  up,  the  blank  is 
allocated 0.3 “time” units (3 implicit steps for DT0 = 0.1) to be loaded with gravity.  At 
the end of gravity loading, a gap of 12mm was created between the upper die and the 
blank,  Figure  11-19.    The  upper  die  is  set  to  be  moved  at  0.3  “time”  units,  closing  the 
gap  caused  by  the  gravity  effect  on  the  blank  (Figure  11-20  left).    An  intermediate 
closing state is shown at t = 0.743 (Figure 11-20 right) while the final completed closing 
is shown in Figure 11-21.  It is noted that the upper die is controlled with displacement 
(VAD = 2)  in  a  shape  of  a  right  triangular  in  the  displacement  versus  “time”  space  as 
defined by load curve #201, and the ID in *CONTACT_AUTO_MOVE is set to “-1”. 
*PARAMETER 
R grvtime       0.3 
R endtime       1.0 
R diemv      145.45 
*CONTROL_TERMINATION 
&endtime 
*CONTROL_IMPLICIT_FORMING 
2,2,100 
*CONTROL_IMPLICIT_GENERAL 
$   IMFLAG       DT0 
         1      0.10  
*CONTROL_ACCURACY 
         1        2 
*CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 
11 
.... 
.... 
.... 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*BOUNDARY_PRESCRIBED_MOTION_RIGID 
$#     pid       dof       vad      lcid        sf       vid     death     birth 
         2         3         2       201 -1.000000         0       0.0     0.000 
*CONTACT_AUTO_MOVE 
$       ID    ContID       VID      LCID     ATIME 
        -1        11        89       201  &grvtime 
*DEFINE_VECTOR 
89,0.0,0.0,0.0,0.0,0.0,-10.0 
*DEFINE_CURVE 
201 
0.0,0.0 
&grvtime,0.0 
1.0,&diemv
Similarly,  “velocity”  controlled  tool  kinematics  is  also  enabled.    In  the  example 
keyword below, the “velocity” profile is ramped up initially and then kept constant.  It 
is noted that the variable VAD in *BOUNDARY is set to “0”, and ID in *CONTACT_-
AUTO_MOVE is set to positive “1” indicating it is a velocity boundary condition. 
*PARAMETER 
R grvtime       0.3 
R tramp       0.001 
R diemv      145.45 
R clsv       1000.0 
*PARAMETER_EXPRESSION 
R tramp1  tramp+gravtime 
R endtime tramp1+(abs(diemv)-0.5*clsv*tramp)/clsv 
*CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 
11 
.... 
.... 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*BOUNDARY_PRESCRIBED_MOTION_RIGID 
$#     pid       dof       vad      lcid        sf       vid     death     birth 
         2         3         0       201 -1.000000         0      0.0      0.000 
*CONTACT_AUTO_MOVE 
$       ID    ContID       VID      LCID     ATIME 
         1        11        89       201  &grvtime 
*DEFINE_VECTOR 
89,0.0,0.0,0.0,0.0,0.0,-10.0 
*DEFINE_CURVE 
201 
0.0,0.0 
0.2,0.0 
&tramp1,&clsv 
&endtime,&clsv 
Example: tool delay in sequential flanging process with explicit dynamic: 
The  following  example  demonstrates  the  use  of  the  variable  OFFSET.    As  shown  in 
Figure 11-22 (left), a total of 5 flange steels are auto-positioned initially according to the 
initial  blank  shape.    Upon  closing  of  the  pressure  pad,  a  first  set  of  4  flanging  steels 
move to home completing the first stage of the stamping process (Figure 11-22 right). 
The gap created by the completion of the first flanging process is closed automatically at 
a time defined using variables ATIME/OFFSET (Figure 11-23 left).  During the second 
stage of the process, flanging steel &flg5pid moves to home completing the final flanging 
(Figure 11-23 right).  An excerpt from the input deck for this model can be found below.  
This  deck  was  created  using  LS-PrePost’s  eZ-Setup  feature  (http://ftp.lstc.com/-
anonymous/outgoing/lsprepost/4.0/metalforming/),  with  two  additional  keywords 
added:*CONTACT_AUTO_MOVE and *DEFINE_VECTOR. 
Flanging  steel  #5  is  set  to  move  in  a  cam  angle  defined  by  vector  #7  following  the 
completion  of  the  flanging  (straight  down)  process  of  flanging  steel  #2.    The  variables 
ATIME  and  OFFSET  in  *CONTACT_AUTO_MOVE  are  both  defined  as  &endtime4, 
which  is  calculated  based  on  the  automatic  positioning  of  tools/blank  using  *CON-
TROL_FORMING_AUTOPOSITION.    At  defined  time,  flanging  steel  #5  ‘jumps’  into
position  to  where  it  just  comes  into  contact  with  the  partially  formed  down-standing 
flange, saving some CPU times (Figure 11-23 left).  Flanging steel #5 continues to move 
to  its  home  position  completing  the  simulation  (Figure  11-23  right).    The  CPU  time 
savings is 27% in this case. 
*KEYWORD   
*PARAMETER 
... 
*PART 
  &flg5pid  &flg5sec  &flg5mid 
... 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
$ Local coordinate system for flanging steel #5 move direction 
*DEFINE_COORDINATE_SYSTEM 
$#     cid        xo        yo        zo        xl        yl        zl 
  &flg5cid  -5.09548   27.6584  -8.98238  -5.43587   26.8608  -9.48034 
$#      xp        yp        zp 
  -5.82509   27.5484  -8.30742 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
$ Auto positioning 
*CONTROL_FORMING_AUTOPOSITION_PARAMETER_SET 
$      SID       CID       DIR      MPID  POSITION   PREMOVE     THICK  PARORDER 
... 
  &flg5sid  &flg5cid         3  &blk1sid        -1             &bthick    flg5mv 
*PART_MOVE 
$    PID            XMOV            YMOV            ZMOV     CID   IFSET 
&flg5sid             0.0             0.0         &flg5mv&flg5cid       1 
... 
*MAT_RIGID 
$      MID        RO         E        PR         N    COUPLE         M     ALIAS 
  &flg5mid 7.830E-09 2.070E+05      0.28 
$      CMO      CON1      CON2 
        -1  &flg5cid    110111 
$LCO or A1        A2        A3        V1        V2        V3 
  &flg5cid 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*CONTACT_AUTO_MOVE 
$       ID    CONTID       VID      LCID     ATIME    OFFSET 
         1         7         7        10  &endtim4  &endtim4 
*DEFINE_VECTOR 
$      VID        XT        YT        ZT        XH        YH        ZH 
         7       0.0       0.0       0.0-0.5931240 0.5930674-0.5444952 
*CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 
$      CID 
         7 
$     SSID      MSID     SSTYP     MSTYP    SBOXID    MBOXID       SPR       MPR 
  &blk1sid  &flg5sid         2         2                             1         1 
$       FS        FD        DC        VC       VDC    PENCHK        BT        DT 
... 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
$                    Tool kinematics 
$  -------------------------closing 
*BOUNDARY_PRESCRIBED_MOTION_RIGID_local 
... 
  &flg5pid         3         0         4       1.0         0  &endtim4 
$  -------------------------flanging 
*BOUNDARY_PRESCRIBED_MOTION_RIGID_local 
... 
  &flg5pid         3         0        10       1.0         0            &endtim4 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*END
*CONTACT 
This  feature  is  implemented  in  LS-DYNA  Revision  64066  and  later  releases.    The 
variable OFFSET is in Revision 77137 and later releases.
Sheet blank
Upper die cavity
Lower binder
Lower punch
Figure 11-18.  Initial parts auto-positioned at t = 0.0. 
12mm gap
Gravity loaded 
sheet blank
Figure 11-19.  Gravity loading on blank at t = 0.2. 
Figure 11-20.  Upper die move down at t = 0.3 closing the gap (left); continue
closing at t = 0.743 (right). 
Figure 11-21.  Closing complete at t = 1.0.
Flanging Steel #2: 0
Flanging steel #5:
&flg5pid
Time = 0 
Time = 0.00954 
ATIME, OFFSET, &endtime4 
Figure  11-22.    A  sequential  flanging  process  (left);  first  set  of  flanging  steels
reaching home (right). 
Time = 0.018743 
Time = 0.026022 
Gap closes.  This happens 
in an “instant,” meaning 
the time step does not 
increment. 
&flg5pid finish 
flanging 
Figure  11-23.    Closing  the  empty  travel  (left);  flanging  steel  &flg5pid
completes flanging process (right).
*CONTACT_COUPLING 
Purpose:    Define  a  coupling  surface  for  MADYMO  to  couple  LS-DYNA  with 
deformable  and  rigid  parts  within  MADYMO.    In  this  interface,  MADYMO  computes 
the contact forces acting on the coupling surface, and LS-DYNA uses these forces in the 
update of the motion of the coupling surface for the next time step.  Contact coupling 
can be used with other coupling options in LS-DYNA. 
2 
3 
4 
5 
6 
7 
8 
  Card 1 
Variable 
1 
ID 
Type 
I 
Default 
required 
Set  Cards.    Include  on  card  for  each  coupled  set.    The  next  "*"  card  terminates  this 
input.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
STYPE 
Type 
I 
I 
Default 
required 
0 
  VARIABLE   
DESCRIPTION
SID 
Set ID for coupling.  See Remark 1 below. 
STYPE 
Set type: 
EQ.0: part set 
EQ.1: shell element set 
EQ.2: solid element set 
EQ.3: thick shell element set
*CONTACT 
1.  Only  one  coupling  surface  can  be  defined.    If  additional  surfaces  are  defined, 
the coupling information will be added to the first definition. 
2.  The  units  and  orientation  can  be  converted  by  using  the  CONTROL_COU-
PLING keyword.  It is not necessary to use the same system of units in MADY-
MO and in LS-DYNA if unit conversion factors are defined.
*CONTACT_ENTITY 
Purpose:  Define a contact entity.  Geometric contact entities treat the impact between a 
deformable body defined as a set of slave nodes or nodes in a shell part set and a rigid 
body.    The  shape  of  the  rigid  body  is  determined  by  attaching  geometric  entities.  
Contact is treated between these geometric entities and the slave nodes using a penalty 
formulation.  The penalty stiffness is optionally maximized within the constraint of the 
Courant  criterion.    As  an  alternative,  a  finite  element  mesh  made  with  shells  can  be 
used  as  geometric  entity.    Also,  axisymmetric  entities  with  arbitrary  shape  made  with 
multi-linear  polygons  are  possible.    The  latter  is  particularly  useful  for  metalforming 
simulations.   
WARNING: If the problem being simulated involves dynamic motion of the entity, care 
should be taken to insure that the inertial properties of the entity are correct.  It may be 
necessary to use the *PART_INERTIA option to specify these properties. 
The data set for *CONTACT_ENTITY consists of 5 cards: 
  Card 1 
1 
2 
3 
4 
Variable 
PID 
GEOTYP 
SSID 
SSTYP 
Type 
I 
I 
I 
Default 
required  required  required
I 
0 
5 
SF 
F 
1. 
6 
DF 
F 
0. 
7 
CF 
F 
0. 
8 
INTORD 
I 
0 
  VARIABLE   
PID 
DESCRIPTION
Part  ID  of  the  rigid  body  to  which  the  geometric  entity  is
attached, see *PART.
GEOTYPE = 1: Infinite Plane
GEOYPE = 2: Sphere
Z'
X'
Y'
GEOYPE = 3: Infinite Cylinder
GEOTYPE = 4: Hyperellipsoid
Figure  11-24.  Contact Entities. 
  VARIABLE   
DESCRIPTION
GEOTYP 
Type of geometric entity: 
EQ.1:  plane, 
EQ.2:  sphere, 
EQ.3:  cylinder, 
EQ.4:  ellipsoid, 
EQ.5: 
torus, 
EQ.6:  CAL3D/MADYMO Plane, see Appendix I, 
EQ.7:  CAL3D/MADYMO Ellipsoid, see Appendix I, 
EQ.8:  VDA surface, see Appendix L, 
EQ.9:  rigid body finite element mesh (shells only), 
EQ.10:  finite plane, 
EQ.11:  load  curve  defining  line  as  surface  profile  of  axisym-
metric rigid bodies.
Y'
Z'
Z'
Y'
X'
g2
GEOTYPE = 5: Torus
GEOTYPE = 10: Finite Plane
X'
g1
Z'
-
axis of symmetry
Load Curve
X'
GEOTYPE = 11: Load Curve
Y'
Figure  11-25.  More contact entities. 
  VARIABLE   
DESCRIPTION
SSID 
Slave set ID, see *SET_NODE_OPTION, *PART, or *SET_PART. 
SSTYP 
Slave set type: 
EQ.0: node set, 
EQ.1: part ID, 
EQ.2: part set ID. 
SF 
DF 
Penalty scale factor.  Useful to scale maximized penalty. 
Damping option, see description for *CONTACT_OPTION: 
EQ.0: no damping, 
GT.0:  viscous  damping  in  percent  of  critical,  e.g.,  20  for  20%
damping, 
LT.0:  DF must be a negative integer.  -DF is the load curve ID 
giving the damping force versus relative normal velocity
.
VARIABLE   
DESCRIPTION
CF 
Coulomb friction coefficient.  See remark 2 below. 
EQ.0: no friction 
GT.0:  constant friction coefficient 
LT.0:  CF must be a negative integer.  -CF is the load curve ID 
giving the friction coefficient versus time. 
INTORD 
Integration  order  (slaved  materials  only).    This  option  is  not
available with entity types 8 and 9 where only nodes are checked:
EQ.0: check nodes only, 
EQ.1: 1 point integration over segments, 
EQ.2: 2 × 2 integration, 
EQ.3: 3 × 3 integration, 
EQ.4: 4 × 4 integration, 
EQ.5: 5 × 5 integration. 
This  option  allows  a  check  of  the  penetration  of  the  rigid  body
into  the  deformable  (slaved)  material.    Then  virtual  nodes  at  the 
location of the integration points are checked. 
Remarks: 
1.  The  optional  load  curves  that  are  defined  for  damping  versus  relative  normal 
velocity and for force versus normal penetration should be defined in the posi-
tive quadrant.  The sign for the damping force depends on the direction of the 
relative velocity and the treatment is symmetric if the damping curve is in the 
positive quadrant.  If the damping force is defined in the negative and positive 
quadrants, the sign of the relative velocity is used in the table look-up. 
2. 
If at any time the friction coefficient is >= 1.0, the force calculation is modified 
to  a  constraint  like  formulation  which  allows  no  sliding.    This  is  only  recom-
mended  for  entities  with  constrained  motion  since  the  mass  of  the  entity  is 
assumed to be infinite.
Variable 
1 
BT 
Type 
F 
2 
DT 
F 
Default 
0. 
1.E+20 
3 
SO 
I 
0 
4 
GO 
I 
0 
*CONTACT_ENTITY 
5 
6 
7 
8 
ITHK 
SPR 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
BT 
DT 
SO 
GO 
Birth time 
Death time 
Flag to use penalty stiffness as in surface-to-surface contact: 
EQ.0: contact entity stiffness formulation, 
EQ.1: surface to surface contact method, 
EQ.2: normal  force  is  computed  via  a  constraint-like  method. 
The contact entity is considered to be infinitely massive,
so this is recommended only for entities with constrained
motion. 
LT.0:  SO must be an integer: 
-SO  is  the  load  curve  ID  giving 
the force versus the normal penetration. 
Flag for automatic meshing of the contact entity for entity types 1-
5  and  10-11.    GO = 1  creates  null  shells  for  visualization  of  the 
contact  entity.        Note  these  shells  have  mass  and  will  affect  the
mass properties of the rigid body PID unless *PART_INERTIA is 
used for the rigid body. 
EQ.0: mesh is not generated, 
EQ.1: mesh is generated. 
ITHK 
Flag for considering thickness for shell slave nodes (applies only
to entity types 1, 2, 3; SSTYP must be set to zero). 
EQ.0: shell thickness is not considered,  
EQ.1: shell thickness is considered,
VARIABLE   
SPR 
  Card 3 
Variable 
1 
XC 
Type 
F 
Default 
0. 
  Card 4 
Variable 
1 
BX 
Type 
F 
Default 
0. 
DESCRIPTION
Include 
interface force files, valid only when SSTYP > 0: 
the  slave  side 
in  *DATABASE_BINARY_INTFOR 
EQ.1: slave side forces included. 
4 
AX 
F 
0. 
5 
AY 
F 
0. 
4 
5 
6 
AZ 
F 
0 
6 
7 
8 
7 
8 
2 
YC 
F 
0. 
2 
BY 
F 
0. 
3 
ZC 
F 
0. 
3 
BZ 
F 
0. 
  VARIABLE   
DESCRIPTION
XC 
YC 
ZC 
AX 
AY 
AZ 
BX 
BY 
𝑥-center, 𝑥𝑐, see remarks below. 
𝑦-center, 𝑦𝑐, see remarks below. 
𝑧-center, 𝑧𝑐.  See remarks below. 
𝑥-direction for local axis 𝐀, 𝐴𝑥, see remarks below. 
y-direction for local axis 𝐀, 𝐴𝑦, see remarks below. 
z-direction for local axis 𝐀, 𝐴𝑧, see remarks below. 
𝑥-direction for local axis 𝐁, Bx, see remarks below. 
𝑦-direction for local axis 𝐁, 𝐵𝑦, see remarks below.
VARIABLE   
DESCRIPTION
BZ 
𝑧-direction for local axis 𝐁, 𝐵𝑧, see remarks below. 
Remarks:: 
1.  The coordinates, (𝑥𝑐, 𝑦𝑐, 𝑧𝑐) are the positions of the local origin of the geometric 
entity  in  global  coordinates.    The  entity’s  local  A-axis  is  determined  by  the 
vector (𝐴𝑥, 𝐴𝑦, 𝐴𝑧) and the local 𝐵-axis by the vector (𝐵𝑥, 𝐵𝑦, 𝐵𝑧). 
2.  Cards  3  and  4  define  a  local  to  global  transformation.    The  geometric  contact 
entities  are  defined  in  a  local  system  and  transformed  into  the  global  system.  
For the  ellipsoid,  this  is  necessary  because  it  has  a  restricted  definition  for  the 
local position.  For the plane, sphere, and cylinder, the entities can be defined in 
the  global  system  and  the  transformation  becomes  (𝑥𝑐, 𝑦𝑐, 𝑧𝑐) = (0,0,0), 
(𝐴𝑥, 𝐴𝑦, 𝐴𝑧) = (1,0,0), and (𝐵𝑥, 𝐵𝑦, 𝐵𝑧) = (0,1,0). 
  Card 5 
1 
Variable 
INOUT 
Type 
Default 
I 
0 
2 
G1 
F 
0. 
3 
G2 
F 
0. 
4 
G3 
F 
0. 
5 
G4 
F 
0. 
6 
G5 
F 
0. 
7 
G6 
F 
0. 
8 
G7 
F 
0. 
  VARIABLE   
INOUT 
G1 
G2 
G3 
G4 
G5 
DESCRIPTION
In-out  flag.    Allows  contact  from  the  inside  or  the  outside
(default) of the entity: 
EQ.0: slave nodes exist outside of the entity, 
EQ.1: slave nodes exist inside the entity. 
Entity coefficient 𝑔1 (CAL3D/MADYMO plane or ellipse number) 
for coupled analysis . 
Entity coefficient 𝑔2, see remarks below. 
Entity coefficient 𝑔3, see remarks below. 
Entity coefficient 𝑔4, see remarks below. 
Entity coefficient 𝑔5, see remarks below.
VARIABLE   
DESCRIPTION
G6 
G7 
Entity coefficient 𝑔6, see remarks below. 
Entity coefficient 𝑔7, see remarks below. 
Remarks: 
Figures  11-24  and  11-25  show  the  definitions  of  the  geometric  contact  entities.    The 
relationships  between  the  entity  coefficients  and  the  Figure  11-25  and  11-24  variables 
are  as  described  below.    Note  that  (𝑃𝑥, 𝑃𝑦, 𝑃𝑧)  defines  a  point  and  (𝑄𝑥, 𝑄𝑦, 𝑄𝑧)  is  a 
direction vector. 
GEOTYP = 1 
𝑔1  =  𝑃𝑥 
𝑔2  =  𝑃𝑦 
𝑔3  =  𝑃𝑧 
𝑔4  =  𝑄𝑥 
𝑔5  =  𝑄𝑦 
𝑔6  =  𝑄𝑧 
𝑔7  =  𝐿 
If  automatic  generation  is  used,  a  square  plane  of  length  L  on  each  edge  is  generated 
which represents the infinite plane.  If generation is inactive, then g7 may be ignored. 
GEOTYP = 2 
GEOTYP = 3 
𝑔1  =  𝑃𝑥 
𝑔2  =  𝑃𝑦 
𝑔3  =  𝑃𝑧 
𝑔1  =  𝑃𝑥 
𝑔2  =  𝑃𝑦 
𝑔3  =  𝑃𝑧 
𝑔4  =  𝑟 
𝑔4  =  𝑄𝑋 
𝑔5  =  𝑄𝑦 
𝑔6  =  𝑄𝑧 
𝑔7  =  𝑟 
If  automatic  generation  is  used,  a  cylinder  of  length  √𝑄x
generated which represents the infinite cylinder. 
2 + 𝑄𝑦
2 + 𝑄z
2  and  radius  r  is 
GEOTYP = 4 
𝑔1  =  𝑃𝑥 
𝑔2  =  𝑃𝑦 
𝑔3  =  𝑃𝑧 
𝑔4  =  𝑎 
𝑔5  =  𝑏 
𝑔6  =  𝑐 
𝑔7  =  𝑛 (order of the ellipsoid)
*CONTACT_ENTITY 
𝑔1  =  Radius of torus 
𝑔2  =  𝑟 
𝑔3  =  number of elements along minor circumference 
𝑔4  =  number of elements along major circumference 
𝑔1  =  Blank thickness (option to override true thickness) 
𝑔2  =  Scale factor for true thickness (optional) 
𝑔3  =  Load curve ID defining thickness versus time.  (optional) 
GEOTYP = 8 
GEOTYP = 9 
𝑔1  =  Shell thickness (option to override true thickness). 
NOTE:  The shell thickness  specification is necessary if the  slave surface is 
generated from solid elements. 
𝑔2  =  Scale factor for true thickness (optional) 
𝑔3  =  Load curve ID defining thickness versus time.  (optional) 
GEOTYP = 10 
𝑔1  =  Length of edge along X′ axis 
𝑔2  =  Length of edge along Y′ axis 
GEOTYP = 11 
𝑔1  =  Load  curve  ID  defining  axisymmetric  surface  profile  about  Z-axis.  
Load  curves  defined  by  the  keywords  *DEFINE_CURVE  or  *DE-
FINE_CURVE_ENTITY can be used. 
𝑔2  =  Number of elements along circumference 
EQ.0:  default set to 10  
𝑔3  =  Number of elements along axis 
EQ.0:  default set to 20 
EQ.-1:  the elements generated from points on the load curve 
𝑔4  =  Number of sub divisions on load curve used to calculate contact 
EQ.0:  default set to 1000
*CONTACT 
Purpose:    Define  contact  interaction  between  the  segment  of  a  GEBOD  dummy  and 
parts  or  nodes  of  the  finite  element  model.    This  implementation  follows  that  of  the 
contact entity, however, it is specialized for the dummies.  Forces may be output using 
the *DATABASE_GCEOUT command.  See *COMPONENT_GEBOD and Appendix N 
for further details. 
Conventional  *CONTACT_OPTION  treatment  (surface-to-surface,  nodes-to-surface, 
etc.)  can  also  be  applied  to  the  segments  of  a  dummy.    To  use  this  approach  it  is  first 
necessary to determine part ID assignments by running the model through LS-DYNA's 
initialization phase. 
The  following  options  are  available  and  refer  to  the  ellipsoids  which  comprise  the 
dummy.    Options  involving  HAND  are  not  applicable  for  the  child  dummy  since  its 
lower arm and hand share a common ellipsoid. 
LOWER_TORSO 
MIDDLE_TORSO 
UPPER_TORSO 
NECK 
HEAD 
RIGHT_LOWER_ARM 
LEFT_HAND 
RIGHT_HAND 
LEFT_UPPER_LEG 
RIGHT_UPPER_LEG 
LEFT_SHOULDER 
LEFT_LOWER_LEG 
RIGHT_SHOULDER 
RIGHT_LOWER_LEG 
LEFT_UPPER_ARM 
RIGHT_UPPER_ARM 
LEFT_LOWER_ARM 
LEFT_FOOT 
RIGHT_FOOT
1 
2 
3 
Variable 
DID 
SSID 
SSTYP 
Type 
I 
I 
I 
4 
SF 
F 
5 
DF 
F 
6 
CF 
F 
Default 
required  required  required
1. 
20. 
0.5 
*CONTACT_GEBOD 
7 
8 
INTORD 
I 
0 
  VARIABLE   
DESCRIPTION
DID 
SSID 
Dummy ID, see *COMPONENT_GEBOD_OPTION. 
Slave set ID, see *SET_NODE_OPTION, *PART, or *SET_PART. 
SSTYP 
Slave set type: 
EQ.0: node set, 
EQ.1: part ID, 
EQ.2: part set ID. 
SF 
DF 
Penalty scale factor.  Useful to scale maximized penalty. 
Damping option, see description for *CONTACT_OPTION: 
EQ.0: no damping, 
GT.0:  viscous  damping  in  percent  of  critical,  e.g.,  20  for  20%
damping, 
LT.0:  DF  must  be  an  integer.    -DF  is  the  load  curve  ID  giving 
the  damping  force  versus  relative  normal  velocity  . 
CF 
Coulomb  friction  coefficient  .    Assumed  to
be constant.
VARIABLE   
DESCRIPTION
INTORD 
Integration order (slaved materials only). 
EQ.0: check nodes only, 
EQ.1: 1 point integration over segments, 
EQ.2: 2 × 2 integration, 
EQ.3: 3 × 3 integration, 
EQ.4: 4 × 4 integration, 
EQ.5: 5 × 5 integration. 
This  option  allows  a  check  of  the  penetration  of  the  dummy
segment  into  the  deformable  (slaved)  material.    Then  virtual
nodes at the location of the integration points are checked. 
4 
5 
6 
7 
8 
  Card 2 
Variable 
1 
BT 
Type 
F 
2 
DT 
F 
Default 
0. 
1.E+20 
3 
SO 
I 
0 
  VARIABLE   
DESCRIPTION
Birth time 
Death time 
Flag to use penalty stiffness as in surface-to-surface contact: 
EQ.0:  contact entity stiffness formulation, 
EQ.1:  surface to surface contact method, 
LT.0:  In this case SO must be an integer.  |SO| gives the load
curve ID giving the force versus the normal penetration.
BT 
DT 
SO 
Remarks: 
1.  The  optional  load  curves  that  are  defined  for  damping  versus  relative  normal 
velocity and for force versus normal penetration should be defined in the posi-
tive quadrant.  The sign for the damping force depends on the direction of the
relative velocity and the treatment is symmetric if the damping curve is in the 
positive quadrant.  If the damping force is defined in the negative and positive 
quadrants, the sign of the relative velocity is used in the table look-up. 
2. 
Insofar  as  these  ellipsoidal  contact  surfaces  are  continuous  and  smooth  it  may 
be necessary to specify Coulomb friction values larger than those typically used 
with faceted contact surfaces.
*CONTACT_GUIDED_CABLE_{OPTION1}_{OPTION2} 
Purpose:  Define a sliding contact that guides 1D elements, such as springs, trusses, and 
beams, along a path defined by a set of nodes.  Only one 1D element can be in contact 
with  any  given  node  in  the  node  set  at  a  given  time.    If  for  some  reason,  a  node  is  in 
contact with multiple 1D elements, one guided contact definition must be used for each 
contact.  The ordering of the nodal points and 1D elements in the input is arbitrary. 
OPTION1 specifies that a part set ID is given with the single option: 
<BLANK> 
SET 
If not used a part ID is assumed. 
OPTION2 specifies that the first card to read defines the heading and ID number of the 
contact interface and takes the single option:   
ID 
Title Card.  Additional card for ID keyword option.  
Title 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CID 
Type 
I 
HEADING 
A70 
  VARIABLE   
DESCRIPTION
CID 
Contact interface ID.  This must be a unique number. 
HEADING 
Interface  descriptor.    It  is  suggested  that  unique  descriptions  be
used.
Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSID 
PID/PSID 
SOFT 
SSFAC 
FRIC 
Type 
I 
I 
Default 
none 
none 
I 
0 
F 
F 
1.0 
none 
  VARIABLE   
DESCRIPTION
NSID 
Node set ID that guides the 1D elements.   
PID/PSID 
Part ID or part set ID if SET is included in the keyword line. 
SOFT 
Flag for soft constraint option.  Set to 1 for soft constraint. 
SSFAC 
Stiffness scale factor for penalty stiffness value.  The default value
is unity.  This applies to SOFT set to 0 and 1. 
FRIC 
Contact friction.
*CONTACT 
Purpose:  Define interior contact for solid elements.  Frequently, when soft materials are 
compressed  under  high  pressure,  the  solid  elements  used  to  discretize  these  materials 
may invert leading to negative volumes and error terminations.  In order to keep these 
elements  from  inverting,  it  is  possible  to  consider  interior  contacts  between  layers  of 
interior surfaces made up of the faces of the solid elements.  Since these interior surfaces 
are  generated  automatically,  the  part  (material)  ID’s  for  the  materials  of  interest  are 
defined here, prior to the interface definitions.  
Define as many cards as necessary.  Input ends at the next * card.  Multiple instances of 
this keyword may appear in the input. 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PSID1 
PSID2 
PSID3 
PSID4 
PSID5 
PSID6 
PSID7 
PSID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
PSID* 
Part set ID  for which interior contact is desired.   
Four attributes should be defined for each part set: 
Attribute 1: 
PSF, penalty scale factor (Default = 1.00). 
Attribute 2: 
Activation  factor,  Fa  (Default = 0.10).    When  the  crushing  of  the 
element reaches Fa times the initial thickness the contact algorithm 
begins to act. 
Attribute 3: 
ED, Optional modulus for interior contact stiffness. 
Attribute 4: 
TYPE, Formulation for interior contact. 
EQ.1.0:  Default, recommended for uniform compression 
EQ.2.0:  Designed to control the combined modes of shear and 
compression.  Works for type 1 brick formulation and 
type 10 tetrahedron formulation.
Define  each  part  set  with  the  *SET_PART_COLUMN  option  to  specify  independent 
attribute values for each part in the part set, 
Remarks: 
The interior penalty is determined by the formula: 
𝐾 =
SLSFAC × PSF × Volume
3⁄ × E
Min. Thickness
where  SLSFAC  is  the  value  specified  on  the  *CONTROL_CONTACT  card  ,  volume  is 
the  volume  of  the  brick  element,    E  is  a  constitutive  modulus,  and  min.    thickness  is 
approximately the thickness of the solid element through its thinnest dimension.   If ED, 
is defined above the interior penalty is then given instead by: 
𝐾 =
3⁄ × ED
Volume
Min. Thickness
where  the  scaling  factors  are  ignored.    Generally,  ED  should  be  taken  as  the  locking 
modulus specified for the foam constitutive model. 
Caution  should  be  observed  when  using  this  option  since  if  the  time  step  size  is  too 
large an instability may result.  The time step size is not affected by the use of interior 
contact.
*CONTACT 
Purpose:  Define rigid surface contact.  The purpose of rigid surface contact is to model 
large  rigid  surfaces,  e.g.,  road  surfaces,  with  nodal  points  and  segments  that  require 
little  storage  and  are  written  out  at  the  beginning  of  the  binary  databases.    The  rigid 
surface motion, which can be optionally prescribed, is defined by a displacement vector 
which  is  written  with  each  output  state.    The  nodal  points  defining  the  rigid  surface 
must  be  defined  in  the  *NODE_RIGID_SURFACE  section  of  this  manual.    These  rigid 
nodal points do not contribute degrees-of-freedom. 
  Card 1 
1 
2 
3 
4 
Variable 
CID 
PSID 
BOXID 
SSID 
Type 
I 
I 
Default 
none 
none 
  Card 2 
1 
2 
I 
0 
3 
5 
FS 
F 
I 
none 
0. 
6 
FD 
F 
0. 
7 
DC 
F 
0. 
8 
VC 
F 
0. 
4 
5 
6 
7 
8 
Variable 
LCIDX 
LCIDY 
LCIDZ 
FSLCID 
FDLCID 
Type 
Default 
I 
0 
  Card 3 
1 
I 
0 
2 
I 
0 
3 
I 
0 
4 
I 
0 
5 
6 
7 
8 
Variable 
SFS 
STTHK 
SFTHK 
XPENE 
BSORT 
CTYPE 
Type 
F 
F 
F 
F 
I 
Default 
1.0 
0.0 
1.0 
4.0 
10 
I 
0 
  VARIABLE   
DESCRIPTION
CID 
Contact interface ID.  This must be a unique number.
VARIABLE   
DESCRIPTION
PSID 
BOXID 
SSID 
FS 
FD 
DC 
VC 
LCIDX 
LCIDY 
Part  set  ID  of  all  parts  that  may  contact  the  rigid  surface.    See
*SET_PART. 
Include  only  nodes  of  the  part  set  that  are  within  the  specified
box,  see  *DEFINE_BOX,  in  contact.    If  BOXID  is  zero,  all  nodes 
from the part set, PSID, will be included in the contact. 
Segment set ID defining the rigid surface.  See *SET_SEGMENT. 
Static coefficient of friction.  The  frictional coefficient is assumed
to  be  dependent  on  the  relative  velocity  𝑣rel  of  the  surfaces  in 
contact, 
𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣. 
If  FSLCID  is  defined,  see  below,  then  FS  is  overwritten  by  the
value from the load curve. 
Dynamic  coefficient  of  friction.    The  frictional  coefficient  is
assumed  to  be  dependent  on  the  relative  velocity  𝑣rel  of  the 
surfaces in contact, 
𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣. 
If  FDLCID  is  defined,  see  below,  then  FD  is  overwritten  by  the
value from the load curve. 
Exponential  decay  coefficient. 
  The  frictional  coefficient  is
assumed  to  be  dependent  on  the  relative  velocity  𝑣rel  of  the 
surfaces in contact 
𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣. 
Coefficient  for  viscous  friction.    This  is  necessary  to  limit  the
friction force to a maximum.  A limiting force is computed, 
𝐹lim = VC × 𝐴cont. 
𝐴cont  being  the  area  of  the  segment  contacted  by  the  node  in
contact.    The  suggested  value  for  VC  is  to  use  the  yield  stress  in 
  where  σo  is  the  yield  stress  of  the  contacted 
shear  VC =
𝜎𝑜
√3
material. 
Load  curve  ID  defining  x-direction  motion.    If  zero,  there  is  no 
motion in the x-coordinate system. 
Load  curve  ID  defining  y-direction  motion.    If  zero,  there  is  no 
motion in the y-coordinate system.
VARIABLE   
DESCRIPTION
Load  curve  ID  defining  z-direction  motion.    If  zero,  there  is  no 
motion in the z-coordinate system. 
Load  curve  ID  defining  the  static  coefficient  of  friction  as  a 
function  of  interface  pressure.      This  option  applies  to  shell
segments only. 
Load  curve  ID  defining  the  dynamic  coefficient  of  friction  as  a
function  of  interface  pressure.    This  option  applies  to  shell
segments only. 
Scale  factor  on  default  slave  penalty  stiffness,  see  also  *CON-
TROL_CONTACT. 
Optional  thickness  for  slave  surface  (overrides  true  thickness).
This  option  applies  to  contact  with  shell,  solid,  and  beam
elements.    True  thickness  is  the  element  thickness  of  the  shell 
elements.  Thickness offsets are not used for solid element unless
this option is specified. 
Scale  factor  for  slave  surface  thickness  (scales  true  thickness).
This  option  applies  only  to  contact  with  shell  elements.    True
thickness is the element thickness of the shell elements. 
Contact  surface  maximum  penetration  check  multiplier.    If  the
penetration  of  a  node  through  the  rigid  surface  exceeds  the
product  of  XPENE  and  the  slave  node  thickness,  the  node  is  set
free. 
EQ.0: default is set to 4.0. 
Number of cycles between bucket sorts.  The default value is set
to  10  but  can  be  much  larger,  e.g.,  50-100,  for  fully  connected 
surfaces. 
The contact formulation.  The default, CTYPE = 0, is equivalent to 
the  ONE_WAY_SURFACE_TO_SURFACE 
formulation,  and 
CTYPE = 1 is a penalty formulation.  If the slave surface belongs
to a rigid body, CTYPE = 1 must be used. 
LCIDZ 
FSLCID 
FDLCID 
SFS 
STTHK 
SFTHK 
XPENE 
BSORT 
CTYPE 
Remarks: 
Thickness offsets do not apply to the rigid surface.  There is no orientation requirement 
for the segments in the rigid surface, and the surface may be assembled from disjoint,
but contiguous, arbitrarily oriented meshes.  With disjoint meshes, the global searches 
must  be  done  frequently,  about  every  10  cycles,  to  ensure  a  smooth  movement  of  a 
slave node between mesh patches.  For fully connected meshes this frequency interval 
can be safely set to 50-200 steps between searches. 
The modified binary database, d3plot, contains the road surface information prior to the 
state data.  This information includes: 
NPDS   =   Total number of rigid surface points in problem. 
NRSC   =   Total  number  of  rigid  surface  contact  segments  summed  over  all 
definitions. 
NSID   =   Number of rigid surface definitions. 
NVELQ   =   Number  of  words  at  the  end  of  each  binary  output  state  defining  the 
rigid surface motion.  This equals 6 × NSID if any rigid surface moves or 
zero if all rigid surfaces are stationary. 
PIDS   =   An  array  equal  in  length  to  NPDS.    This  array  defines  the  ID  for  each 
point in the road surface. 
XC   =   An array equal in length to 3 × NPDS.  This array defines the global x, y, 
and z coordinates of each point. 
For each road surface define the following NSID sets of data: 
ID   =   Rigid surface ID. 
NS   =   Number of segments in rigid surface. 
IXRS   =   An array equal in length to 4 × NS.  This is the connectivity of the rigid 
surface in the internal numbering system. 
At the end of each state, 6 × NVELQ words of information are written.  For each road 
surface  the  x,  y,  and  z  displacements  and  velocities  are  written.    If  the  road  surface  is 
fixed,  a  null  vector  should  be  output.    Skip  this  section  if  NVELQ = 0.    LS-PrePost 
currently displays rigid surfaces and animates their motion.
*CONTACT 
Purpose:  Define one-dimensional slide lines for rebar in concrete. 
  Card 1 
1 
2 
3 
4 
Variable 
NSIDS 
NSIDM 
ERR 
SIGC 
Type 
I 
I 
F 
Default 
none 
none 
0. 
F 
0. 
5 
GB 
F 
0. 
6 
7 
8 
SMAX 
EXP 
F 
0. 
F 
0. 
  VARIABLE   
DESCRIPTION
NSIDS 
Nodal set ID for the slave nodes, see *SET_NODE. 
NSIDM 
Nodal set ID for the master nodes, see *SET_NODE. 
ERR 
SIGC 
GB 
External radius of rebar 
Unconfined compressive strength of concrete, 𝑓𝑐 
Bond shear modulus 
SMAX 
Maximum shear strain 
EXP 
Exponent in damage curve 
Remarks: 
With  this  option  the  concrete  is  defined  with  solid  elements  and  the  rebar  with  truss 
elements,  each  with  their  own  unique  set  of  nodal  points.      A  string  of  spatially 
consecutive  nodes,  called  slave  nodes,  related  to  the  truss  elements  may  slide  along 
another  string  of  spatially  consecutive  nodes,  called  master  nodes,  related  to  the  solid 
elements.  The sliding commences after the rebar debonds. 
The bond between the rebar and concrete is assumed to be elastic perfectly plastic.  The 
maximum allowable slip strain is given as: 
𝑢max = SMAX × 𝑒−EXP×𝐷 
where 𝐷 is the damage parameter 𝐷𝑛+1 = 𝐷𝑛 + Δ𝑢.  The shear force, acting on area 𝐴𝑆, 
at time 𝑛 + 1 is given as: 
𝑓𝑛+1 = min[𝑓𝑛 − GB × 𝐴𝑠 × Δ𝑢, GB × 𝐴𝑠 × 𝑢max]
*CONTACT_2D_OPTION1_{OPTION2}_{OPTION3} 
Purpose:    Define  a  2-dimensional  contact  interface  or  slide  line.    This  option  is  to  be 
used  with  2D  solid  and  shell  elements  using  the  plane  stress,  plane  strain  or 
axisymmetric formulations, see *SECTION_SHELL and SECTION_BEAM. 
All the 2D contacts are supported in SMP.    Only *CONTACT_2D_AUTOMATIC_SIN-
GLE_SURFACE  and  *CONTACT_2D_AUTOMATIC_SURFACE_TO_SURFACE  are 
supported for MPP. 
OPTION1  specifies  the  contact  type.    The  following  options  activate  kinematic 
constraints and should be used with deformable materials only, but may be used with 
rigid  bodies  if  the  rigid  body  is  the  master  surface  and  all  rigid  body  motions  are 
prescribed.    Kinematic  constraints  are  recommended  for  high  pressure  hydrodynamic 
applications. 
SLIDING_ONLY 
TIED_SLIDING 
SLIDING_VOIDS 
AUTOMATIC_TIED_ONE_WAY 
The following option uses both kinematic constraints and penalty constraints. 
AUTOMATIC_TIED 
The  following  options  are  penalty  based.    These  methods  have  no  rigid-material 
limitations.  They are recommended for lower pressure solid mechanics applications. 
PENALTY_FRICTION 
PENALTY 
AUTOMATIC_SINGLE_SURFACE 
AUTOMATIC_SINGLE_SURFACE_MORTAR  
AUTOMATIC_SURFACE_TO_SURFACE 
AUTOMATIC_SURFACE_TO_SURFACE_MORTAR 
AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE 
AUTOMATIC_SURFACE_IN_CONTINUUM 
For these contact types, the Mortar contact is available only for implicit and only supported 
in SMP at the moment.
The following options are used for SPH particles in contact with 2D solid elements (2D 
shell  elements  are  not  supported  currently)  using  the  plane  stress,  plane  strain  or 
axisymmetric formulations: 
NODE_TO_SOLID 
NODE_TO_SOLID_TIED 
The  following  option  is  used  to  measure  contact  forces  that  are  reported  as  RCFORC 
output. 
FORCE_TRANSDUCER 
OPTION2 specifies a thermal contact and takes the single option: 
THERMAL 
Only  the  AUTOMATIC  contact  options:  SINGLE_SURFACE,  SURFACE_TO_SUR-
FACE,  and  ONE_WAY_SURFACE_TO_SURFACE  may  be  used  with  the  THERMAL 
option. 
OPTION3 specifies that the first card to read defines the title and ID number of contact 
interface and takes the single option: 
TITLE 
Title Card.  Additional card for the TITLE keyword potion. 
Title 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CID 
Type 
I 
NAME 
A70 
The 2D contact may be divided into 3 groups, each with a unique input format. 
1.  The  first  group  were  adopted  from  LS-DYNA2D  and  originated  in  the  public 
domain version of DYNA2D from the Lawrence Livermore National Laborato-
ry.    Contact  surfaces  are  specified  as  ordered  sets  of  nodes.    These  sets  define 
either  contact  surfaces  or  slide  lines.    The  keyword  options  for  the  first  group 
are: 
SLIDING_ONLY 
TIED_SLIDING
SLIDING_VOIDS 
PENALTY_FRICTION 
PENALTY 
NOTE:  TIED_SLIDING,  PENALTY_FRICTION  and  PE-
NALTY  options  are  not  recommended  since  there 
are  automatic  options  in  the  second  group  that  are 
easier to use and provide the same functionality. 
2.  The second group contains the automatic contacts.  These contact surfaces may 
be  defined  using  part  sets  or  unordered  node  sets.    Segment  orientations  are 
determined automatically.  The keywords for these are: 
AUTOMATIC_SINGLE_SURFACE 
AUTOMATIC_SINGLE_SURFACE_MORTAR 
AUTOMATIC_SURFACE_TO_SURFACE 
AUTOMATIC_SURFACE_TO_SURFACE_MORTAR 
AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE 
AUTOMATIC_SURFACE_IN_CONTINUUM 
AUTOMATIC_TIED 
AUTOMATIC_TIED_ONE_WAY 
FORCE_TRANSDUCER 
3.  The third group is used for SPH particles in contact with continuum elements: 
NODE_TO_SOLID 
NODE_TO_SOLID_TIED 
Each  of  the  3  groups  has  a  section  below  with  a  description  of  input  and  additional 
remarks.
*CONTACT_2D_[SLIDING, TIED, & PENALTY]_OPTION 
This section documents the *CONTACT_2D variations derived from DYNA2D: 
SLIDING_ONLY 
TIED_SLIDING 
SLIDING_VOIDS 
PENALTY_FRICTION 
PENALTY. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
MSID 
TBIRTH 
TDEATH 
Type 
I 
I 
F 
F 
Default 
none 
none 
0. 
1.e20 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EXT_PAS  THETA1 
THETA2 
TOL_IG 
PEN 
TOLOFF 
FRCSCL  ONEWAY 
Type 
I 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
0.001 
0.1 
0.025 
0.010 
0.0 
Friction Card.  Additional card for the PENALTY_FRICTION keyword option. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FRIC 
FRIC_L 
FRIC_H 
FRIC_S 
Type 
F 
F 
F
VARIABLE   
SSID 
DESCRIPTION
Nodal  set  ID  for  the  slave  nodes,  see  *SET_NODE.    The  slave 
surface must be to the left of the master surface. 
MSID 
Nodal set ID for the master nodes, see *SET_NODE.   
TBIRTH 
Birth time for contact. 
TDEATH 
Death time for contact. 
EXT_PAS 
Slide line extension bypass option. 
EQ.0: extensions are use 
EQ.1: extensions are not used 
THETA1 
Angle in degrees of slide line extension at first master node. 
EQ.0: extension remains tangent to first master segment. 
THETA2 
Angle in degrees of slide line extension at last master node. 
EQ.0: extension remains tangent to last master segment. 
TOL_IG 
Tolerance for determining initial gaps. 
EQ.0.0: default set to 0.001 
PEN 
Scale factor or penalty. 
EQ.0.0: default set to 0.10 
TOLOFF 
Tolerance  for  stiffness  insertion  for  implicit  solution  only.    The
contact stiffness is inserted when a node approaches a segment a
distance equal to the segment length multiplied by TOLOFF.  The
stiffness  is  increased  as  the  node  moves  closer  with  the  full 
stiffness being used when the nodal point finally makes contact. 
EQ.0.0: default set to 0.025. 
FRCSCL 
Scale factor for the interface friction. 
EQ.0.0: default set to 0.010
Better.  This is the
extensionwhen m17
is included.
Poor.  This is the extension if m17 is
excluded from the slideline definition.
This extension may spuriously interact
with slave nodes s1 and s2.  
m9
m16
m15
m17
m1
m2
m3
m4
m5
m6m6
s1
s2
s3
s4
s5
s6
s7
s8
s9
s10
s15
s16
s17
s18
s19
s20
s21
s22
s23
m10
m11
m12
m13
s11
s12 s13 s14 s24
m7
m8
m14m14
Slide Lines
14
11
12
13
14
24
m s m s m s
17
24
23
22
21
20
19
18
17
16
15
14
13
12
11
19
15
16
10
11
Master Slide Line
Slave Slide line
Slide line Extension
Master surface: nodes m1 - m17
Slave surface: nodes s1 - s24
Figure 11-26.  Slide line Example.  Note: (1) as recommend, for 90° angles each
facet is assigned a distinct slide line; (2) the master slide line is more coarsely
meshed; (3) the slave is to the left of the master (following the node ordering,
see inset table); (4) as shown for slave nodes 1 and 2 it is important the slide
line extension does not spuriously come into contact. 
  VARIABLE   
ONEWAY 
DESCRIPTION
Flag for one way treatment.  If set to 1.0 the nodal points on the
slave surface are constrained to the master surface.  This option is
generally recommended if the master surface is rigid. 
EQ.1.0: activate one way treatment. 
FRIC 
Coefficient of friction 
FRIC_L 
Coefficient of friction at low velocity.
VARIABLE   
DESCRIPTION
FRIC_H 
Coefficient of friction at high velocity. 
FRIC_S 
Friction factor for shear. 
Remarks: 
The SLIDING_ONLY option is a two-surface method based on a kinematic formulation.  
The two surfaces are allowed to slide arbitrarily large distances without friction, but are 
not permitted to separate or interpenetrate.  Surfaces should be initially in contact.  This 
option  performs  well  when  extremely  high  interface  pressures  are  present.    The  more 
coarsely meshed surface should be chosen as the master surface for best performance. 
The TIED_SLIDING option joins two parts of a mesh with differing mesh refinement.  It 
is a kinematic formulation so the more coarsely meshed surface should be chosen as the 
master. 
The SLIDING_VOIDS option is a kinematic formulation without friction which permits 
two surfaces to separate if tensile forces develop across the interface.  The surfaces may 
be initially in contact or initially separated. 
The  PENALTY_FRICTION  and  PENATLY  options  are  penalty  formulations  so  the 
designation  of  master  and  slave  surfaces  is  not  important.    The  two  bodies  may  be 
initially  separate  or  in  contact.    A  rate-dependent  Coulomb  friction  model  is  available 
for PENALTY_FRICTION. 
Consider two slide line surfaces in  contact.  It is necessary to designate one as a slave 
surface and the other as a master surface.  Nodal points defining the slave surface are 
called  slave  nodes,  and  similarly,  nodes  defining  the  master  surface  are  called  master 
nodes.  Each slave-master surface combination is referred to as a slide line. 
Many  potential  problems  with  the  options  can  be  avoided  by  observing the  following 
precautions: 
•  Metallic materials should contain the master surface along high explosive-metal 
interfaces. 
•  SLIDING_ONLY  type  slide  lines  are  appropriate  along  high  explosive-metal 
interfaces.  The penalty formulation is not recommended along such interfaces. 
•  If  one  surface  is  more  finely  zoned,  it  should  be  used  as  the  slave  surface.    If 
penalty  slide  lines  are  used,  PENALTY  and  PENALTY_FRICTION,  then  the 
slave-master distinction is irrelevant. 
•  A slave node may have more than one master segment, and may be included as 
a member of a master segment if a slide line intersection is defined.
•  Angles in the master side of a slide line that approach 90° must be avoided. 
Whenever such angles exist in a master surface, two or more slide lines should be 
defined.    This  procedure  is  illustrated  in  Figure  11-26.    An  exception  for  the 
foregoing  rule  arises  if  the  surfaces  are  tied.    In  this  case,  only  one  slide  line  is 
needed. 
•  Whenever two surfaces are in contact, the smaller of the two surfaces should be 
used as the slave surface.  For example, in modeling a missile impacting a wall, 
the contact surface on the missile should be used as the slave surface. 
•  Care  should  be  used  when  defining  a  master  surface  to  prevent  the  extension 
from interacting with the solution.  In Figures 11-26 and 11-27,  slide line exten-
sions are shown.
With extension
of slide lines turned
off, the slave nodes
move down the
inner walls as shown.
Master
surface
Slave
surface
With extension and proper
slide line definition, elements
behave as expected.
Slide line
extension
Extended slide lines do not
allow for penetration
Figure  11-27.    With  and  without  extension.    Extensions  may  be  turned  off  by
setting EXT_PAS (card 2), but, when turned off, slave nodes may “leak” out as
shown in the upper version of the figure.
*CONTACT_2D_[AUTOMATIC, & FORCE_TRANSDUCER]_OPTION 
This section documents the following variations of *CONTACT_2D: 
AUTOMATIC_SINGLE_SURFACE 
AUTOMATIC_SINGLE_SURFACE_MORTAR  
AUTOMATIC_SURFACE_TO_SURFACE 
AUTOMATIC_SURFACE_TO_SURFACE_MORTAR  
AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE 
AUTOMATIC_SURFACE_IN_CONTINUUM 
AUTOMATIC_TIED 
AUTOMATIC_TIED_ONE_WAY 
FORCE_TRANSDUCER 
  Card 1 
1 
2 
3 
4 
Variable 
SIDS 
SIDM 
SFACT 
FREQ 
Type 
I 
I 
F 
I 
Default 
none 
none 
1.0 
50 
8 
5 
FS 
F 
0. 
6 
FD 
F 
0. 
7 
DC 
F 
0. 
Remarks 
1 
  Card 2 
1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TBIRTH 
TDEATH 
SOS 
SOM 
NDS 
NDM 
COF 
INIT 
Type 
F 
F 
F 
F 
Default 
0. 
1.e20 
1.0 
1.0 
Remarks 
3 
3 
I 
0 
2 
I 
0 
2 
I 
0 
I 
0
Automatic Thermal Card.  Additional card for keywords with both the AUTOMATIC 
and THERMAL options.  For example, *CONTACT_2D_AUTOMATIC_..._THERMAL_
..... 
  Card 3 
Variable 
Type 
1 
K 
F 
2 
RAD 
F 
3 
H 
F 
4 
5 
6 
7 
8 
LMIN 
LMAX 
CHLM 
BC_FLAG 
Default 
none 
none 
none 
none 
none 
1.0 
F 
F 
F 
I 
0 
Automatic Optional Card 1.  Optional card for the AUTOMATIC keyword option. 
  Card 4 
Variable 
1 
VC 
2 
3 
4 
5 
6 
7 
8 
VDC 
IPF 
SLIDE 
ISTIFF 
TIEDGAP 
IGAPCL 
TIETYP 
Type 
F 
F 
Default 
0. 
10.0 
I 
0 
I 
0 
7 
I 
0 
8 
R 
9 
I 
0 
I 
0 
9 
Remarks 
  VARIABLE   
SIDS 
SIDM 
DESCRIPTION
Set  ID  to  define  the  slave  surface.    If  SIDS > 0,  a  part  set  is 
assumed, see *SET_PART.  If SIDS < 0, a node set with ID equal to 
the absolute value of SIDS is assumed, see *SET_NODE. 
Set  ID  to  define  the  master  surface.    If  SIDM > 0,  a  part  set  is 
assumed, see *SET_PART.  If SIDM < 0, a node set with ID equal 
to  the  absolute  value  of  SIDM  is  assumed,  see  *SET_NODE.    Do 
not define for single surface contact. 
SFACT 
Scale factor for the penalty force stiffness. 
FREQ 
Search frequency.  The number of timesteps between bucket sorts.
For  implicit  contact  this  parameter  is  ignored  and  the  search
frequency is 1.
FS 
FD 
EQ.0: default set to 50. 
Static coefficient of friction.  The  frictional coefficient is assumed 
to  be  dependent  on  the  relative  velocity  𝑣rel  of  the  surfaces  in 
contact according to the relation given by: 
𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣𝑟𝑒𝑙∣. 
Dynamic  coefficient  of  friction.    The  frictional  coefficient  is
assumed  to  be  dependent  on  the  relative  velocity  𝑣rel  of  the 
surfaces in contact 
𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣. 
This parameter does not apply to Mortar contact. 
DC 
Exponential  decay  coefficient. 
  The  frictional  coefficient  is 
assumed  to  be  dependent  on  the  relative  velocity  𝑣rel  of  the 
surfaces in contact  
𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣. 
This parameter does not apply to Mortar contact. 
TBIRTH 
Birth time for contact. 
TDEATH 
Death time for contact. 
SOS 
Surface offset from midline for 2D shells of slave surface 
EQ.0.0: default to 1. 
GT.0.0:  scale factor applied to actual thickness 
LT.0.0:  absolute value is used as the offset 
SOM 
Surface offset from midline for 2D shells of master surface 
EQ.0: default to 1. 
GT.0:  scale factor applied to actual thickness 
LT.0:  absolute value is used as the offset
NDS 
Normal direction flag for 2D shells of slave surface 
EQ.0:  Normal direction is determined automatically 
EQ.1:  Normal direction is in the positive direction 
EQ.-1:  Normal direction is in the negative direction 
NDM 
Normal direction flag for 2D shells of master surface 
EQ.0:  Normal direction is determined automatically 
EQ.1:  Normal direction is in the positive direction 
EQ.-1:  Normal direction is in the negative direction 
COF 
Closing/Opening flag for implicit contact 
EQ.0: Recommended  for  most  problem  where  gaps  are  only
closing. 
EQ.1: Recommended when gaps are opening to avoid sticking.
This parameter does not apply to Mortar contact. 
INIT 
Special processing during initialization 
EQ.0: No special processing. 
EQ.1: Forming option. 
K 
RAD 
Thermal conductivity (k) of fluid between the slide surfaces.  If a 
gap  with  a  thickness  𝑙gap  exists  between  the  slide  surfaces,  then 
the  conductance  due  to  thermal  conductivity  between  the  slide 
surfaces is 
ℎcond =
𝑙gap
Note that LS- DYNA calculates 𝑙gap based on deformation. 
Radiation  factor,  f,  between  the  slide  surfaces.    A  radiant-heat-
transfer  coefficient  (ℎrad)  is  calculated  .    If  a  gap  exists  between  the  slide  surfaces,  then  the
contact conductance is calculated by 
ℎ = ℎcond + ℎrad
H 
Heat  transfer  conductance  (ℎ𝑐𝑜𝑛𝑡)  for  closed  gaps.    Use  this  heat 
transfer conductance for gaps in the range 
0 ≤ 𝑙gap ≤ 𝑙min
LMIN 
LMAX 
CHLM 
where 𝑙min is GCRIT defined below. 
Critical  gap  (𝑙min),  use  the  heat  transfer  conductance  defined 
(HTC) for gap thicknesses less than this value. 
No thermal contact if gap is greater than this value (𝑙max). 
Is a multiplier used on the element characteristic distance for the 
search  routine.    The  characteristic  length  is  the  largest  interface
surface element diagonal. 
EQ.0: Default set to 1.0 
BC_FLAG 
Thermal boundary condition flag 
EQ.0: thermal  boundary  conditions  are  on  when  parts  are  in
contact 
EQ.1: thermal  boundary  conditions  are  off  when  parts  are  in
contact 
VC 
Coefficient  for  viscous  friction.    This  is  used  to  limit  the  friction
force to a maximum.  A limiting force is computed 
𝐹lim = VC × 𝐴cont. 
𝐴cont  being  the  area  of  contacted  between  segments.    The
suggested value for VC is to use the yield stress in shear: 
VC =
𝜎𝑜
√3
where 𝜎𝑜 is the yield stress of the contacted material. 
VDC 
Viscous  damping  coefficient  in  percent  of  critical  for  explicit
contact.  This parameter does not apply to Mortar contact. 
IPF 
Initial penetration flag for explicit contact. 
EQ.0: Allow initial penetrations to remain 
EQ.1: Push apart initially penetrated surfaces 
SLIDE 
Sliding option. 
EQ.0: Off 
EQ.1: On 
ISTIFF 
Stiffness scaling option. 
EQ.0: Use default option.
EQ.1: Scale  stiffness  using  segment  masses  and  explicit  time
step (default for explicit contact) 
EQ.2: Scale  stiffness  using  segment  stiffness  and  dimensions
(default for implicit contact) 
TIEDGAP 
Search gap for tied contacts. 
EQ.0: Default, use 1% of the master segment length 
GT.0:  Use the input value 
LT.0:  Use –TIEDGAP % of the master segment length. 
IGAPCL 
Flag to close gaps in tied contact 
EQ.0: Default, allow gaps to remain 
EQ.1: Move slave nodes to master segment to close gaps 
TIETYP 
Flag to control constraint type of tied contact 
EQ.0: Default, use kinematic constraints when possible 
EQ.1: Use only penalty type constraints 
Remarks: 
1.  The  SINGLE_SURFACE,  SURFACE_TO_SURFACE,  and  ONE_WAY_SUR-
FACE_TO_SURFACE  options  use  penalty  forces  to  prevent  penetration  be-
tween 2D shell elements and external faces of 2D continuum elements.  Contact 
surfaces are defined using SIDS and SIDM to reference either part sets or node 
sets.  If part sets are used, all elements and continuum faces of the parts in the 
set are included in contact.  If node sets are used, elements or continuum faces 
that  have  both  nodes  in  the  set  are  included  in  the  contact  surface.    The  SIN-
GLE_SURFACE option  uses  only  the  slave set  and  checks  for  contact  between 
all  elements  and  continuum  faces  in  the  set.    If  SSID  is  blank  or  zero,  contact 
will  be  checked  for  all  elements  and  continuum  faces  in  the  model.    With  the 
other options, both SSID and MSID are required. 
2.  The FORCE_TRANSDUCER option should be used in conjunction with at least 
one AUTOMATIC contact options.  It does nothing to prevent penetration, but 
measures  the  forces  generated  by  other  contact  definitions.    The  FORCE_-
TRANSDUCER  option  uses  only  SIDS,  and  optionally  SIDM.    If  only  SIDS  is 
defined,  the  force  transducer  measures  the  resultant  contact  force  on  all  the 
elements and continuum faces in the slave surface.  If both SIDS and SIDM are 
defined,  then  the  force  transducer  measures  contact  forces  between  the  ele-
ments and continuum faces in the slave surface and master surface.  The meas-
ured  forces  are  included  in  the  rcforc  output.    In  the  case  of  an  axisymmetric 
analysis, values output to rcforc and ncforc are in units of force per radian (this 
includes both shell types 14 and 15). 
3.  By default, the normal direction of 2D shell elements is evaluated automatically 
for  SINGLE_SURFACE,  SURFACE_TO_SURFACE  and  ONE_WAY_SUR-
FACE_TO_SURFACE  contact.    The  user  can  override  the  automatic  algorithm 
using NDS or NDM and contact will occur with the positive or negative face of 
the element. 
4.  By default, the true thickness of 2D shell elements is taken into account for the 
SURFACE_TO_SURFACE,  SINGLE_SURFACE,  and  ONE_WAY_SURFACE_-
TO_SURFACE options.  The user can override the true thickness by using SOS 
and SOM.  If the surface offset is reduced to a small value, the automatic nor-
mal  direction  algorithm  may  fail,  so  it  is  best  to  specify  the  normal  direction 
using NDS or NDM. 
5.  For all AUTOMATIC contact options, eroding materials are treated by default.  
At present, subcycling is not possible. 
6.  The  INIT  parameter  activates  a  forming  option  that    is  intended  for  implicit 
solutions  of  thin  solid  parts  when  back  side  segments  may  interfere  with  the 
solution.    It  automatically  removes  back  side  segments  during  initialization.  
Alternatively,  the  user  can  input  INIT = 0,  and  use  node  set  input  to  limit  the 
contact interface to just the front of a thin part. 
7.  For the thermal option: 
ℎ = ℎcont, if the gap thickness is 0 ≤ 𝑙gap ≤ 𝑙min 
ℎ = ℎcond + ℎrad, if the gap thickness is 𝑙min ≤ 𝑙gap ≤ 𝑙max 
ℎ = 0, if the gap thickness is 𝑙gap > 𝑙max 
8.  The  SLIDE  parameter activates  a  sliding option  which  uses  additional  logic  to 
improve sliding when surfaces in contact have kinks or corners.  This option is 
off by default. 
9.  The ISTIFF option allows control of the equation used in calculating the penalty 
stiffness.    For  backward  compatibility,  the  default  values  are  different  for  im-
plicit  and  explicit  solutions.    When  ISTIFF = 1  is  used,  the  explicit  time  step 
appears  in  the  stiffness  equation  regardless  if  the  calculation  is  implicit  or  ex-
plicit. 
10.  The  TIED_ONE_WAY  contact  creates  two  degree  of  freedom  translational 
kinematic  constraints  to  nodes  on  the  slave  surface  which  are  initially  located
on  or  near  master  segments.    The  TIED  option  creates  kinematic  constraints 
between slave nodes and master segments, and also creates penalty constraints 
between master nodes and slave segments.  With either contact option, a kine-
matic  constraint  may  be  switched  to  penalty  if  there  is  a  conflict  with  another 
constraint.  The TIEDGAP parameter determines the maximum normal distance 
from  a  segment  to  a  node  for  a  constraint  to  be  formed.    Nodes  will  not  be 
moved  to  eliminate  an  initial  gap,  and  the  initial  gap  will  be  maintained 
throughout the calculation.  If TIETYP = 1, then only penalty constraints will be 
used. 
11.  Note  that  the  SURFACE_IN_CONTINUUM  option  has  been  deprecated  in 
favor of the *CONSTRAINED_LAGRANGE_IN_SOLID keyword which allows 
coupling between fluids and structures.  However, this option is maintained to 
provide backward compatibility for existing data. 
For  the  SURFACE_IN_CONTINUUM  option,  penalty  forces  prevent  the  flow 
of slave element material (the continuum) through the master surfaces.  Flow of 
the  continuum  tangent  to  the  surface  is  permitted.    Only  2D  solid  parts  are 
permitted in the slave part set.  Both 2D solid and 2D shell parts are permitted 
in  the  master  part  set.    Flow  through  2D  shell  elements  is  prevented  in  both 
directions by default.  If NDM is set to ±1, flow in the direction of the normal is 
permitted.  Thickness of 2D shell elements is ignored. 
12.  When using the SURFACE_IN_CONTINUUM option, there is no need to mesh 
the  continuum  around  the  structure  because  contact  is  not  with  continuum 
nodes  but  with  material  in  the  interior  of  the  continuum  elements.    The  algo-
rithm  works  well  for  Eulerian  or  ALE  elements  since  the  structure  does  not 
interfere  with remeshing.    However,  a  structure  will  usually  not  penetrate  the 
surface  of  an  ALE  continuum  since  the  nodes  are  Lagrangian  normal  to  the 
surface.   Therefore, if  using an ALE  fluid, the structure should be initially im-
mersed in the fluid and remain immersed throughout the calculation.  Penetrat-
ing the surface of an Eulerian continuum is not a problem. 
13.  The  Mortar  contact  (MORTAR)  is  available  for  implicit  calculations  in  SMP 
(MPP  not  supported).    The  apparent  behavior  compared  to  the  non-Mortar 
contact is very similar, the difference lies in details concerning the constitutive 
relation (contact stress vs relative motion of contact surfaces) and the kinemat-
ics  (the  relative  motion  of  contact  surfaces  as  function  of  nodal  coordinates).  
Mortar contact is designed for continuity and smoothness that is beneficial for 
an  implicit  solution  scheme,  and  is  intended  to  enhance  robustness  in  such  a 
context.  For details regarding the 2D Mortar contact, see the LS-DYNA Theory 
Manual.
*CONTACT_2D_NODE_TO_SOLID_OPTION 
This section documents the following variations of *CONTACT_2D: 
NODE_TO_SOLID 
NODE_TO_SOLID_TIED 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
MSID 
TBIRTH 
TDEATH 
Type 
I 
I 
F 
F 
Default 
none 
None 
0. 
1.e20 
3 
VC 
F 
4 
5 
OFFD 
PEN 
F 
F 
6 
FS 
F 
7 
FD 
F 
8 
DC 
F 
0.0 
0.0 
1.0/0.1 
0.0 
0.0 
0.0 
  Card 2 
1 
2 
Variable 
SOFT 
Type 
Default 
I 
0 
  VARIABLE   
SSID 
DESCRIPTION
Nodal  set  ID  or  part  set  ID  for  the  slave  nodes,  If  SSID > 0,  a 
nodal set ID is assumed, If SSID < 0 a part set ID is assumed. 
MSID 
Master part set ID.  MSID < 0 since only part set is allowed. 
TBIRTH 
Birth time for contact. 
TDEATH 
Death time for contact.
VARIABLE   
DESCRIPTION
SOFT 
Soft constraint option: 
EQ.0:  penalty formulation, 
EQ.1:  soft constraint formulation. 
The  soft  constraint  may  be  necessary  if  the  material  constants  of
the  parts  in  contact  have  a  wide  variation  in  the  elastic  bulk
moduli.    In  the  soft  constraint  option,  the  interface  stiffness  is
based  on  the  nodal  mass  and  the  global  time  step  size.    The  soft 
for  axisymmetric
is  also  recommended 
constraint  option 
simulations. 
VC 
Coefficient  for  viscous  friction.    This  is  used  to  limit  the  friction
force to a maximum.  A limiting force is computed 
𝐹lim = VC × 𝐴cont. 
𝐴cont  being  the  area  of  contacted  between  segments.    The
suggested value for VC is to use the yield stress in shear: 
VC =
𝜎𝑜
√3
where 𝜎𝑜 is the yield stress of the contacted material. 
OFFD 
Contact offset distance for slave nodes (SPH particles), not for tie
contact  right  now.    Recommended  to  be  half  of  the  original
particle spacing in contact direction. 
PEN 
Scale factor for penalty. 
FS 
FD 
EQ.0.0: default set to 1.0 for penalty formulation, or 0.1 for soft 
constraint formulation. 
Static coefficient of friction.  The  frictional coefficient is assumed
to  be  dependent  on  the  relative  velocity  𝑣rel  of  the  surfaces  in 
contact according to the relationship given by: 
𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣. 
Dynamic  coefficient  of  friction.    The  frictional  coefficient  is
assumed  to  be  dependent  on  the  relative  velocity  𝑣rel  of  the 
surfaces in contact 
𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣.
DESCRIPTION
Exponential  decay  coefficient. 
  The  frictional  coefficient  is
assumed  to  be  dependent  on  the  relative  velocity  vrel  of  the 
surfaces in contact 
𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣. 
  VARIABLE   
DC 
Remarks: 
NODE_TO_SOLID contact is a penalty based contact type used only for SPH particles 
with  solid  elements  using  the  plane  stress,  plane  strain  or  axisymmetric  formulation.  
NODE_TO_SOLID_TIED  contact  is  used  only  for  SPH  particles  tied  with  solid  
elements, an offset of distance h (smooth length) is adopted for each SPH particle.
The  keyword  control  cards  are  optional  and  can  be  used  to  change  defaults  activate 
solution  options  such  as  mass  scaling  adaptive  remeshing  and  an  implicit  solution 
however it is advisable to define the CONTROL_TERMINATION card.  The ordering 
of  the  control  cards  in  the  input  file  is  arbitrary.    To  avoid  ambiguities  define  no 
more than one control card of each type.  The following control cards are organized in 
alphabetical order 
*CONTROL_ACCURACY 
*CONTROL_ACOUSTIC 
*CONTROL_ADAPSTEP 
*CONTROL_ADAPTIVE 
*CONTROL_ADAPTIVE_CURVE 
*CONTROL_ALE 
*CONTROL_BULK_VISCOSITY 
*CONTROL_CHECK_SHELL 
*CONTROL_COARSEN 
*CONTROL_CONTACT 
*CONTROL_COUPLING 
*CONTROL_CPM 
*CONTROL_CPU 
*CONTROL_DEBUG 
*CONTROL_DISCRETE_ELEMENT 
*CONTROL_DYNAMIC_RELAXATION 
*CONTROL_EFG 
*CONTROL_ENERGY 
*CONTROL_EXPLICIT_THERMAL_ALE_COUPLING 
*CONTROL_EXPLICIT_THERMAL_BOUNDARY
*CONTROL_EXPLICIT_THERMAL_INITIAL 
*CONTROL_EXPLICIT_THERMAL_OUTPUT 
*CONTROL_EXPLICIT_THERMAL_PROPERTIES 
*CONTROL_EXPLICIT_THERMAL_SOLVER 
*CONTROL_EXPLOSIVE_SHADOW 
*CONTROL_FORMING_AUTOCHECK 
*CONTROL_FORMING_AUTONET 
*CONTROL_FORMING_AUTOPOSITION_PARAMETER 
*CONTROL_FORMING_BESTFIT 
*CONTROL_FORMING_INITIAL_THICKNESS 
*CONTROL_FORMING_MAXID 
*CONTROL_FORMING_ONESTEP 
*CONTROL_FORMING_OUTPUT 
*CONTROL_FORMING_PARAMETER_READ 
*CONTROL_FORMING_POSITION 
*CONTROL_FORMING_PREBENDING 
*CONTROL_FORMING_PROJECTION 
*CONTROL_FORMING_REMOVE_ADAPTIVE_CONSTRAINTS 
*CONTROL_FORMING_SCRAP_FALL 
*CONTROL_FORMING_SHELL_TO_TSHELL 
*CONTROL_FORMING_STONING 
*CONTROL_FORMING_TEMPLATE 
*CONTROL_FORMING_TIPPING 
*CONTROL_FORMING_TOLERANC 
*CONTROL_FORMING_TRAVEL
*CONTROL_FORMING_TRIMMING 
*CONTROL_FORMING_UNFLANGING 
*CONTROL_FORMING_USER 
*CONTROL_FREQUENCY_DOMAIN 
*CONTROL_HOURGLASS_{OPTION} 
*CONTROL_IMPLICIT_AUTO 
*CONTROL_IMPLICIT_BUCKLE 
*CONTROL_IMPLICIT_CONSISTENT_MASS 
*CONTROL_IMPLICIT_DYNAMICS 
*CONTROL_IMPLICIT_EIGENVALUE 
*CONTROL_IMPLICIT_FORMING 
*CONTROL_IMPLICIT_GENERAL 
*CONTROL_IMPLICIT_INERTIA_RELIEF 
*CONTROL_IMPLICIT_JOINTS 
*CONTROL_IMPLICIT_MODAL_DYNAMIC 
*CONTROL_IMPLICIT_MODAL_DYNAMIC_DAMPING_{OPTION} 
*CONTROL_IMPLICIT_MODAL_DYNAMIC_MODE_{OPTION} 
*CONTROL_IMPLICIT_MODES_{OPTION} 
*CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS 
*CONTROL_IMPLICIT_SOLUTION 
*CONTROL_IMPLICIT_SOLVER 
*CONTROL_IMPLICIT_STABILIZATION 
*CONTROL_IMPLICIT_STATIC_CONDENSATION_{OPTION} 
*CONTROL_IMPLICIT_TERMINATION 
*CONTROL_MAT
*CONTROL_MPP_DECOMPOSITION_ARRANGE_PARTS_{OPTION} 
*CONTROL_MPP_DECOMPOSITION_AUTOMATIC 
*CONTROL_MPP_DECOMPOSITION_BAGREF 
*CONTROL_MPP_DECOMPOSITION_CHECK_SPEED 
*CONTROL_MPP_DECOMPOSITION_CONTACT_DISTRIBUTE 
*CONTROL_MPP_DECOMPOSITION_CONTACT_ISOLATE 
*CONTROL_MPP_DECOMPOSITION_DISTRIBUTE_ALE_ELEMENTS 
*CONTROL_MPP_DECOMPOSITION_DISTRIBUTE_SPH_ELEMENTS 
*CONTROL_MPP_DECOMPOSITION_ELCOST 
*CONTROL_MPP_DECOMPOSITION_FILE 
*CONTROL_MPP_DECOMPOSITION_METHOD 
*CONTROL_MPP_DECOMPOSITION_NUMPROC 
*CONTROL_MPP_DECOMPOSITION_OUTDECOMP 
*CONTROL_MPP_DECOMPOSITION_PARTS_DISTRIBUTE 
*CONTROL_MPP_DECOMPOSITION_PARTSET_DISTRIBUTE_{OPTION} 
*CONTROL_MPP_DECOMPOSITION_RCBLOG 
*CONTROL_MPP_DECOMPOSITION_SCALE_CONTACT_COST 
*CONTROL_MPP_DECOMPOSITION_SCALE_FACTOR_SPH 
*CONTROL_MPP_DECOMPOSITION_SHOW 
*CONTROL_MPP_DECOMPOSITION_TRANSFORMATION 
*CONTROL_MPP_IO_BINOUTONLY 
*CONTROL_MPP_IO_LSTC_REDUCE 
*CONTROL_MPP_IO_NOBEAMOUT 
*CONTROL_MPP_IO_NOD3DUMP 
*CONTROL_MPP_IO_NODUMP
*CONTROL_MPP_IO_NOFULL 
*CONTROL_MPP_IO_SWAPBYTES 
*CONTROL_MPP_MATERIAL_MODEL_DRIVER 
*CONTROL_MPP_PFILE 
*CONTROL_NONLOCAL 
*CONTROL_OUTPUT 
*CONTROL_PARALLEL 
*CONTROL_PORE_FLUID 
*CONTROL_REFINE_ALE 
*CONTROL_REFINE_ALE2D 
*CONTROL_REFINE_MPP_DISTRIBUTION 
*CONTROL_REFINE_SHELL 
*CONTROL_REFINE_SOLID 
*CONTROL_REMESHING 
*CONTROL_REQUIRE_REVISION 
*CONTROL_RIGID 
*CONTROL_SHELL 
*CONTROL_SOLID 
*CONTROL_SOLUTION 
*CONTROL_SPH 
*CONTROL_SPOTWELD_BEAM 
*CONTROL_START 
*CONTROL_STAGED_CONSTRUCTION 
*CONTROL_STEADY_STATE_ROLLING 
*CONTROL_STRUCTURED_{OPTION}
*CONTROL_TERMINATION 
*CONTROL_THERMAL_EIGENVALUE 
*CONTROL_THERMAL_NONLINEAR 
*CONTROL_THERMAL_SOLVER 
*CONTROL_THERMAL_TIMESTEP 
*CONTROL_TIMESTEP 
*CONTROL_UNITS 
LS-DYNA’s  implicit  mode  may  be  activated in  two  ways.    Using the  *CONTROL_IM-
PLICIT_GENERAL  keyword,  a  simulation  may  be  flagged  to  run  entirely  in  implicit 
mode.    Alternatively,  an  explicit  simulation  may  be  seamlessly  switched  into  implicit 
mode  at  the  termination  time  using  the  *INTERFACE_SPRINGBACK_SEAMLESS 
keyword.    The  seamless  switching  feature  is  intended  to  simplify  metal  forming 
springback calculations, where the forming phase can be run in explicit mode, followed 
immediately  by  an  implicit  static  springback  simulation.    In  case  of  difficulty,  restart 
capability  is  supported.    Eight  keywords  are  available  to  support  implicit  analysis.  
Default values are carefully selected to minimize input necessary for most simulations.  
These are summarized below: 
*CONTROL_IMPLICIT_GENERAL 
Activates implicit mode, selects time step size. 
*CONTROL_IMPLICIT_INERTIA_RELIEF 
Allows linear analysis of models with rigid body modes. 
*CONTROL_IMPLICIT_SOLVER 
Selects parameters for solving system of linear equations [K]{x}={f}. 
*CONTROL_IMPLICIT_SOLUTION 
Selects linear or nonlinear solution method, convergence tolerances. 
*CONTROL_IMPLICIT_AUTO 
Activates automatic time step control. 
*CONTROL_IMPLICIT_DYNAMICS 
Activates and controls dynamic implicit solution using Newmark method. 
*CONTROL_IMPLICIT_EIGENVALUE 
Activates and controls eigenvalue analysis.
Activates and controls computation of constraint and attachment modes. 
*CONTROL_IMPLICIT_STABILIZATION 
Activates and controls artificial stabilization for multi-step spring back.
*CONTROL_ACCURACY 
Purpose:  Define control parameters that can improve the accuracy of the calculation. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OSU 
INN 
PIDOSU 
IACC 
Type 
I 
I 
I 
I 
Default 
0 (off) 
optional
0 (off) 
  VARIABLE   
OSU 
DESCRIPTION
Global  flag  for  2nd  order  objective  stress  updates  .    Generally,  for  explicit  calculations  only  those  parts
undergoing large rotations, such as rolling tires, need this option.
Objective stress updates can be activated for a subset of part IDs
by defining the part set in columns 21-30. 
EQ.0: Off (default) 
EQ.1: On 
INN 
Invariant  node  numbering  for  shell  and  solid  elements.    . 
EQ.-4:  On  for  both  shell  and  solid  elements  except  triangular 
shells 
EQ.-2:  On for shell elements except triangular shells 
EQ.1:  Off (default for explicit) 
EQ.2:  On  for  shell  and  thick  shell  elements  (default  for
implicit) 
EQ.3:  On for solid elements 
EQ.4:  On for shell, thick shell, and solid elements 
PIDOSU 
Part set ID for objective stress updates.  If this part set ID is given
only  those  part  IDs  listed  will  use  the  objective  stress  update;
therefore, OSU is ignored.
DESCRIPTION
Implicit  accuracy 
turns  on  some  specific  accuracy
considerations  in  implicit  analysis  at  an  extra  CPU  cost.    See 
Remark 4.  
flag, 
EQ.0:  Off (default) 
EQ.1:  On 
  VARIABLE   
IACC 
Remarks: 
1.  Second  Order  Objective  Stress  Update.    Second  order  objective  stress 
updates  are  occasionally  necessary.    Some  examples  include  spinning  bodies 
such  as  turbine  blades  in  a  jet  engine,  high  velocity  impacts  generating  large 
strains  in  a  few  time  steps,  and  large  time  step  sizes  due  to  mass  scaling  in 
metal  forming.    There  is  a  significantly added  cost  which  is  due  in  part to the 
added  cost  of  the  second  order  terms  in  the  stress  update  when  the  Jaumann 
rate is used and the need to compute the strain-displacement matrix at the mid-
point geometry.  This option is available for one point brick elements, the selec-
tive-reduced  integrated  brick  element  which  uses  eight  integration  points,  the 
fully  integrated  plane  strain  and  axisymmetric  volume  weighted  (type  15)  2D 
solid  elements,  the  thick  shell  elements, and  the  following  shell  elements:    Be-
lytschko-Tsay,  Belytschko-Tsay  with  warping  stiffness,  Belytschko-Chiang-
Wong, S/R Hughes-Liu, and the type 16 fully integrated shell element. 
2. 
Invariant  Node  Numbering  for  Shell  Elements.    Invariant  node  numbering 
for  shell  and  thick  shell  elements  affects  the  choice  of  the  local  element  shell 
coordinate  system.    The  orientation  of  the  default  local  coordinate  system  is 
based on the shell normal vector and the direction of the 1-2 side of the element.  
If  the  element  numbering  is  permuted,  the  results  will  change  in  irregularly 
shaped elements.  With invariant node numbering, permuting the nodes shifts 
the local system by an exact multiple of 90 degrees.  In spite of its higher costs 
[<5%],  the  invariant  local  system  is  recommended  for  several  reasons.    First, 
element forces are nearly independent of node sequencing; secondly, the hour-
glass  modes  will  not  substantially  affect  the  material  directions;  and,  finally, 
stable calculations over long time periods are achievable.  The INN parameter 
has  no  effect  on  thick  shell  form  2  which  is  always  invariant  and  thick  shell 
from 3 which is never invariant. 
3. 
Invariant  Node  Numbering  for  Solid  Elements.    Invariant  node  numbering 
for solid elements is available for anisotropic materials only.  This option has no 
effect  on  solid  elements  of  isotropic  material.    This  option  is  recommended 
when solid elements of anisotropic material undergo significant deformation.
4. 
Implicit  Calculations.    All  other  things  being  equal,  a  single  time  step  of  an 
implicit analysis usually involves a larger time increment and deformation than 
an  explicit  analysis.    Many  of  the  algorithms  in  LS-DYNA  have  been  heavily 
optimized for explicit analysis in ways that are inappropriate for implicit analy-
sis.    While  an  implicit  analysis,  by  default,  invokes  many  measures  to  ensure 
accuracy, certain corrections associated with unusual applications or with large 
computational expense are invoked only by setting IACC = 1.  A list of features 
that are included with this option follows. 
a)  Strongly  objective  treatment  of  some  tied  contact 
interfaces,  see 
*CONTACT. 
b)  Fully iterative treatment of some piecewise linear plasticity materials, see 
*MAT_PIECEWISE_LINEAR_PLASTICITY 
*MAT_MODIFIED_-
PIECEWISE_LINEAR_PLASTICITY,  including  smooth  decay  of  stresses 
down to zero when including failure. 
and 
c)  Strong  objective  treatment  of  some  elements  in  the  context  of  large  rota-
tions, applies to shell element types -16, 16 and 4, beam element types 1, 2 
and  9,  and  solid  element  types  -2,  -1,  1,  2  and  16.    The  superposed  rigid 
body  motion  is  subtracted  from  these  elements  before  evaluating  the  re-
sponse which significantly reduces the presence of spurious strains.
*CONTROL 
Purpose:  Define control parameters for transient acoustic solutions. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MACDVP 
Type 
Default 
I 
0 
  VARIABLE   
MACDVP 
Remarks: 
DESCRIPTION
Calculate  the  nodal  displacements  and  velocities  of  *MAT_-
ACOUSTIC  volume  elements  for  inclusion  in  d3plot  and  time-
history files. 
EQ.0:  Acoustic nodal motions will not be calculated 
EQ.1:  Acoustic nodal motions will be calculated 
1. 
*MAT_ACOUSTIC volume elements (ELFORM = 8 and ELFORM = 14) use the 
displacement  potential  as  the  fundamental  unknown.    The  infinitesimal  mo-
tions  of  these  acoustic  nodes  can  be  found  from  the  gradient  of  the  displace-
ment  and  velocity  potentials.    This  is  purely  a  post-processing  endeavor  and 
has no effect on the predicted pressures and structural response.  It will howev-
er  roughly  double  the  cost  of  the  acoustic  solution  and  for  that  reason  is  not 
done by default. 
2.  The  acoustic  theory  underpinning  *MAT_ACOUSTIC  volume  elements 
presumes infinitesimal motions.  In the presence of larger motions the pressure 
calculations  will  proceed  regardless,  but  the  calculation  of  acoustic  nodal  mo-
tions can then be unreliable.
*CONTROL_ADAPSTEP 
Purpose:    Define  control  parameters  for  contact  interface  force  update  during  each 
adaptive cycle. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FACTIN 
DFACTR 
Type 
F 
F 
Default 
1.0 
0.01 
  VARIABLE   
FACTIN 
DESCRIPTION
Initial  relaxation  factor  for  contact  force  during  each  adaptive
remesh.  To turn this option off set FACTIN = 1.0.  Unless stability 
problems  occur  in  the  contact,  FACTIN = 1.0  is  recommended 
since this option can create some numerical noise in the resultant 
tooling forces.  A typical value for this parameter is 0.10. 
DFACTR 
Incremental  increase  of  FACTIN  during  each  time  step  after  the
adaptive step.  FACTIN is not allowed to exceed unity.  A typical
value might be 0.01. 
Remarks: 
1.  This command applies to contact with thickness offsets including contact types: 
*CONTACT_FORMING_…_ 
*CONTACT_NODES_TO_SURFACE_ 
*CONTACT_SURFACE_TO_SURFACE 
*CONTACT_ONE_WAY_SURFACE_TO_SURFACE.
*CONTROL 
Purpose:    Activate  adaptive  meshing.    The  parts  which  are  adaptively  meshed  are 
defined  by  ADPOPT  under  *PART.    Note  that  “sandwiched”  part’s  adaptivity  is 
available  when  the  variable  IFSAND  is  set  to  “1”  and  applies  to  ADPOPT = 1  and  2 
only.    Other  related  keywords  include:  *CONTROL_ADAPTIVE_CURVE,  *DEFINE_-
CURVE_TRIM  (with  variable  TCTOL),  *DEFINE_BOX_ADAPTIVE  (moving  adaptive 
box), and *DEFINE_CURVE_BOX_ADAPTIVITY.  This keword is applicable to neither 
hyperelastic materials nor any material model based on a Total Lagrangian formulation. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  ADPFREQ  ADPTOL 
ADPOPT  MAXLVL 
TBIRTH 
TDEATH 
LCADP 
IOFLAG 
Type 
F 
F 
Default 
none 
1020 
I 
1 
I 
3 
F 
F 
0.0 
1020 
I 
0 
I 
0 
Remaining cards are optional.† 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ADPSIZE  ADPASS 
IREFLG 
ADPENE 
ADPTH  MEMORY  ORIENT  MAXEL 
Type 
F 
Default 
  Card 3 
1 
I 
0 
2 
I 
0 
3 
F 
F 
I 
I 
I 
0.0 
inactive inactive 
0 
inactive
4 
5 
6 
7 
8 
Variable 
IADPN90 
IADPGH 
NCFREQ 
IADPCL 
ADPCTL 
CBIRTH 
CDEATH 
LCLVL 
Type 
Default 
I 
0 
I 
0 
I 
none 
I 
1 
F 
F 
F 
F 
none 
0.0 
1020
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CNLA 
MMM2D  ADPERR  D3TRACE 
IFSAND 
Type 
Default 
F 
0 
  VARIABLE   
ADPFREQ 
ADPTOL 
I 
0 
I 
0 
I 
0 
I 
0 
DESCRIPTION
Time interval between adaptive refinements, see Figures 12-2 and 
12-1. 
Adaptive  error  tolerance  in  degrees  for  ADPOPT  set  to  1  or  2
below.    If  ADPOPT  is  set  to  8,  ADPTOL  is  the  characteristic
element size. 
ADPOPT 
Adaptive options: 
EQ.1: angle change in degrees per adaptive refinement relative 
to the surrounding shells for each shell to be refined. 
EQ.2: total angle change in degrees relative to the surrounding
shells  for  each  shell  to  be  refined.    For  example,  if  the
adptol = 5 degrees, the shell will be refined to the second
level  when  the  total  angle  change  reaches  5  degrees.
When  the  angle  change  is  10  degrees  the  shell  will  be
refined to the third level. 
EQ.4: adapts  when  the  shell  error  in  the  energy  norm,  Δ𝑒, 
exceeds  ADPTOL/100  times  the  mean  energy  norm
within the part, which is estimated as: 
Δ𝑒 = (∫
Ω𝑒
2⁄
‖Δ𝜎‖2
𝑑Ω
)
where  𝐸  is  Young's  modulus.    The    error  of  the  stresses
Δ𝜎 is defined as the difference between the the recovered
solution  𝜎 ⋆  and 
i.e. 
Δ𝜎 ≡ 𝜎 ⋆ − 𝜎 ℎ.    Various  recovery  techniques  for  𝜎 ⋆  and 
error  estimators  for  Δ𝑒  are  defined  by  ADPERR.    This 
options works for shell types 2, 4, 16, 18, 20. 
the  numerical  solution,  𝜎 ℎ 
EQ.7: 3D  r-adaptive  remeshing  for  solid  elements.    Solid
element type 13, a tetrahedron, and 3-D EFG type 41 and 
42, are used in the adaptive remeshing process.  A com-
VARIABLE   
DESCRIPTION
pletely  new  mesh  is  generated  which  is  initialized  from
the  old  mesh  using  a  least  squares  approximation.    The
mesh size is currently based on the minimum and maxi-
mum  edge 
the  *CONTROL_-
REMESHING  keyword  input.    This  option  remains 
under development, and, we are not sure of its reliability
on complex geometries. 
lengths  defined  on 
EQ.8: 2D  𝑟-adaptive  remeshing  for  axisymmetric  and  plane
strain  continuum  elements.    A  completely  new  mesh  is
generated which is initialized from the old mesh using a 
least squares approximation.  The mesh size is currently
based on the value, ADPTOL, which gives the character-
istic  element  size.    This  option  is  based  on  earlier  work
by Dick and Harris [1992].  If ADPTOL is negative, then 
self-contacting material will not be merged together.  The 
self-merging  is  often  preferred  since  it  eliminates  sharp
folds in the boundary; however, if the sharp fold is being
simulated unexpected results are generated. 
Maximum  number  of  refinement  levels.    Values  of  1,  2,  3,  4,  … 
allow  a  maximum  of  1,  4,  16,  64,  …  shells,  respectively,  to  be
created  for  each  original  shell.    The  refinement  level  can  be
overridden  by  *DEFINE_BOX_ADAPTIVE,  or  *DEFINE_SET_-
ADAPTIVE. 
Birth  time  at  which  the  adaptive  remeshing  begins,  see  Figures 
12-2 and 12-1. 
Death  time  at  which  the  adaptive  remeshing  ends,  see  Figures 
12-2 and 12-1. 
Adaptive interval is changed as a function of time given by load
curve  ID,  LCADP.    If  this  option  is  nonzero,  the  ADPFREQ  will
be  replaced  by  LCADP.    The  𝑥-axis  is  time  and  the  𝑦-axis  is  the 
varied adaptive time interval. 
Flag  to  generate  adaptive  mesh  at  exit  including  *NODE,  *ELE-
MENT_SHELL_THICKNESS,  *BOUNDARY_option,  and  *CON-
STRAINED_ADAPTIVITY, to be saved in the file, adapt.msh. 
EQ.1: generate ℎ-adapted mesh. 
MAXLVL 
TBIRTH 
TDEATH 
LCADP 
IOFLAG 
ADPSIZE 
Minimum shell size to be adapted based on element edge length.
If undefined the edge length limit is ignored.
(cid:98)(cid:106)(cid:29)(cid:97)(cid:106)(cid:89) (cid:70)(cid:51)(cid:51)(cid:85) (cid:106)(cid:67)(cid:76)(cid:51) (cid:64)(cid:67)(cid:99)(cid:65)
(cid:106)(cid:82)(cid:97)(cid:119) (cid:67)(cid:78) (cid:47)(cid:107)(cid:84)(cid:72)(cid:81)(cid:105)(cid:89)
(cid:50)(cid:113)(cid:82)(cid:73)(cid:113)(cid:51) (cid:56)(cid:97)(cid:82)(cid:76) (cid:486) (cid:106)(cid:82)
(cid:486)(cid:3718) (cid:30) (cid:486) (cid:12) (cid:34)(cid:37)(cid:49)(cid:39)(cid:51)(cid:38)(cid:50)(cid:15)
(cid:99)(cid:51)(cid:106)(cid:45) (cid:486) (cid:30) (cid:486)(cid:3718)
(cid:106)(cid:51)(cid:97)(cid:67)(cid:76)(cid:67)(cid:78)(cid:29)(cid:106)(cid:67)(cid:82)(cid:78)
(cid:106)(cid:67)(cid:76)(cid:51) (cid:97)(cid:51)(cid:29)(cid:44)(cid:64)(cid:51)(cid:48)(cid:93)
(cid:119)(cid:51)(cid:99)
(cid:50)(cid:113)(cid:82)(cid:73)(cid:113)(cid:51) (cid:56)(cid:97)(cid:82)(cid:76) (cid:486)
(cid:106)(cid:82) (cid:486)(cid:3718) (cid:82)(cid:78) (cid:97)(cid:51)(cid:126)(cid:78)(cid:51)(cid:48)
(cid:76)(cid:51)(cid:99)(cid:64)(cid:89)
(cid:105)(cid:51)(cid:97)(cid:76)(cid:67)(cid:78)(cid:29)(cid:106)(cid:51)(cid:89)
(cid:114)(cid:97)(cid:67)(cid:106)(cid:51) (cid:106)(cid:82)
(cid:47)(cid:107)(cid:84)(cid:72)(cid:81)(cid:105)(cid:89)
(cid:78)(cid:82)
(cid:70)(cid:83)(cid:83)(cid:80)(cid:83) (cid:29)
(cid:85)(cid:80)(cid:77)(cid:70)(cid:83)(cid:66)(cid:79)(cid:68)(cid:70)(cid:93)
(cid:78)(cid:82)
(cid:96)(cid:51)(cid:126)(cid:78)(cid:51) (cid:76)(cid:51)(cid:99)(cid:64) (cid:29)(cid:106) (cid:106)(cid:67)(cid:76)(cid:51)
(cid:486) (cid:86)(cid:78)(cid:82)(cid:106) (cid:486)(cid:3718)(cid:87)(cid:89) (cid:47)(cid:82)(cid:78)(cid:533)(cid:106) (cid:99)(cid:29)(cid:113)(cid:51)
(cid:110)(cid:78)(cid:97)(cid:51)(cid:126)(cid:78)(cid:51)(cid:48) (cid:99)(cid:82)(cid:73)(cid:110)(cid:106)(cid:67)(cid:82)(cid:78)(cid:89)
(cid:119)(cid:51)(cid:99)
(cid:99)(cid:51)(cid:106)(cid:45) (cid:486) (cid:30) (cid:486)(cid:3718)
write
re(cid:1)ne 
time
22
tbirth
11 33
ADPFREQ
end
time
Figure 12-1.  Flowchart for ADPASS = 0.  While this option is sometimes more
accurate,  ADPASS = 1  is  much  less  expensive  and  recommended  when  used
with ADPENE. 
  VARIABLE   
DESCRIPTION
LT.0: absolute  value  defines 
the  minimum  characteristic
element length to be adapted based on square root of the
element  area,  i.e.,  instead  of  comparing  the  shortest  ele-
ment edge with ADPSIZE, it compares the square root of 
the element area with |ADPSIZE| whenever ADPSIZE is
defined by a negative value. 
ADPASS 
One or two pass flag for ℎ-adaptivity: 
EQ.0: two pass adaptivity as shown in Figure 12-2. 
EQ.1: one pass adaptivity as shown in Figure 12-1. 
IREFLG 
Uniform refinement level.  A value of 1, 2, 3 … allow 4, 16, 64 …
shells, respectively, to be created uniformly for each original shell.
If negative, |IREFLG| is taken as a load curve ID.  With the curve
time
tbirth
(cid:98)(cid:106)(cid:29)(cid:97)(cid:106)(cid:89) (cid:70)(cid:51)(cid:51)(cid:85) (cid:106)(cid:67)(cid:76)(cid:51) (cid:64)(cid:67)(cid:99)(cid:65)
(cid:106)(cid:82)(cid:97)(cid:119) (cid:67)(cid:78) (cid:47)(cid:107)(cid:84)(cid:72)(cid:81)(cid:105)(cid:89)
(cid:51)(cid:113)(cid:82)(cid:73)(cid:113)(cid:51) (cid:106)(cid:67)(cid:76)(cid:51) (cid:106)(cid:82)
(cid:486) (cid:12) (cid:34)(cid:37)(cid:49)(cid:39)(cid:51)(cid:38)(cid:50)
ADPFREQ
(cid:119)(cid:51)(cid:99)
(cid:105)(cid:51)(cid:97)(cid:76)(cid:67)(cid:78)(cid:29)(cid:106)(cid:51)(cid:89)
(cid:114)(cid:97)(cid:67)(cid:106)(cid:51) (cid:106)(cid:82)
(cid:47)(cid:107)(cid:84)(cid:72)(cid:81)(cid:105)(cid:89)
(cid:106)(cid:51)(cid:97)(cid:67)(cid:76)(cid:67)(cid:78)(cid:29)(cid:106)(cid:67)(cid:82)(cid:78)
(cid:106)(cid:67)(cid:76)(cid:51) (cid:97)(cid:51)(cid:29)(cid:44)(cid:64)(cid:51)(cid:48)(cid:93)
(cid:78)(cid:82)
(cid:97)(cid:51)(cid:126)(cid:78)(cid:51) (cid:76)(cid:51)(cid:99)(cid:64)(cid:46) (cid:67)(cid:56)
(cid:97)(cid:51)(cid:92)(cid:110)(cid:67)(cid:97)(cid:51)(cid:48)
re(cid:1)ne 
re(cid:1)ne 
re(cid:1)ne 
re(cid:1)ne 
end
time
Figure 12-2.  Flow chart for ADPASS = 1.  This algorithm may be summarized
as,    “periodically  refine”    This  method  is  recommended  over  ADPASS = 0
when used with ADPENE, which implements look ahead. 
  VARIABLE   
DESCRIPTION
option,  the  abscissa  values  define  the  refinement  time,  and  the
ordinate  values  define  the  minimum  element  size.    Only  one
refinement level is performed per time step.  An advantage of the
load  curve  option  is  that  the  mesh  is  adapted  to  honor  the
minimum element size, but with the uniform option, IREFLG > 0, 
this is not possible. 
NOTE: If  the  element  size  defined  with  *DEFINE_CURVE  is 
positive,  the  element  size  will  override  the  element  size  defined
with  *CONTROL_ADAPTIVE  and  *DEFINE_SET_ADAPTIVE.
Also,  if  the  element  size  defined  with  *DEFINE_CURVE  is 
negative the element size is used for refinement only. 
For shell, ℎ-adapt the mesh when the FORMING contact surfaces
approach or penetrate the tooling surface depending on whether 
is  positive  (approach)  or  negative 
the  value  of  ADPENE 
(penetrates),  respectively.    The  tooling  adaptive  refinement  is
based on the curvature of the tooling.  If ADPENE is positive the
takes  place;
refinement  generally  occurs  before  contact 
ADPENE
VARIABLE   
DESCRIPTION
consequently, it is possible that the parameter ADPASS can be set
to 1 in invoke the one pass adaptivity. 
For three dimensions 𝑟-adaptive solid remeshing (ADPOPT = 2 in 
*PART),  the  mesh  refinement  is  based  on  the  curvature  of  the
tooling when ADPENE is positive.  See Remark 6.  
ADPTH 
EQ.0.0: This parameter is ignored 
GT.0.0:  Absolute  shell  thickness  level  below  which  adaptive
remeshing should began. 
LT.0.0:  Element  thickness  reduction  ratio.    If  the  ratio  of  the 
element  thickness  to  the  original  element  thickness  is 
less than  1.0+ADPTHK, the element will be refined. 
This option works only if ADPTOL is nonzero.  If thickness based
adaptive  remeshing  is  desired  without  angle  changes,  then,  set
ADPTOL to a large angle. 
MEMORY 
the  machine  and  operating  system 
This  flag  can  have  two  meanings  depending  on  whether  the
memory  environmental  variable  is  or  is  not  set.    The  command 
"setenv  LSTC_MEMORY  auto"  (or  for  bourne  shell  “export 
LSTC_MEMORY=auto”) sets the memory environmental variable 
which  causes LS-DYNA to expand memory automatically.  Note
that  automatic  memory  expansion  is  not  always  100%  reliable 
depending  on 
level;
consequently,  it  is  not  yet  the  default.    To  see  if  this  is  set  on  a
particular machine type the command "env".  If the environmen-
tal  variable  is  not  set  then  when  memory  usage  reaches  this 
percentage,  MEMORY,  further  adaptivity  is  prevented  to  avoid
exceeding  the  memory  specified  at  execution  time.    Caution  is
necessary  since  memory  usage  is  checked  after  each  adaptive
step,  and,  if  the  memory  usage  increases  by  more  than  the
residual  percentage,  100-PERCENT, 
calculation  will 
terminate. 
If  the  memory  environmental  variable  is  set  then  when  the 
number  of  words  of  memory  allocated  reaches  or  exceeds  this
value, MEMORY, further adaptivity is stopped. 
the 
ORIENT 
This option applies to the FORMING contact option only.  If this 
flag is set to one (1), the user orientation for the contact interface
is  used.    If  this  flag  is  set  to  zero  (0),  LS-DYNA  sets  the  global 
orientation of the contact surface the first time a potential contact
is observed after the birth time.   If slave nodes are found on both
sides  of  the  contact  surface,  the  orientation  is  set  based  on  the
VARIABLE   
DESCRIPTION
principle  of  "majority  rules".    Experience  has  shown  that  this
principle is not always reliable. 
MAXEL 
Adaptivity is stopped if this number of shells is exceeded. 
IADPN90 
Maximum  number  of  shells  covering  90  degree  of  radii.    See
Remark 5. 
IADPGH 
Fission flag for neighbor splitting. 
EQ.0: split all neighbor shells 
EQ.1: do not split neighbor shells 
NCFREQ 
IADPCL 
ADPCTL 
CBIRTH 
Frequency of fission to fusion steps.  For example, if NCFREQ = 4, 
then  fusion  will  occur  on  the  fourth,  eighth,  twelfth,  etc.,  fission
steps,  respectively.    If  this  option  is  used  NCFREQ > 1  is 
recommended. 
Fusion  will  not  occur  until  the  fission  level  reaches  IADPCL. 
Therefore, if IADPCL = 2, MAXLVL = 5, any shell can be split into 
256 shells.  If the surface flattens out, the number of elements will
be reduced if the fusion option is active, i.e., the 256 elements can
be fused and reduced to 16. 
Adaptivity  error  tolerance  in  degrees  for  activating  fusion.    It
follows the same rules as ADPOPT above. 
Birth  time  for  adaptive  fusion.    If  ADPENE > 0,  look-ahead 
adaptivity  is  active.    In  this  case,  fission,  based  on  local  tool
curvature,  will  occur  while  the  blank  is  still  relatively  flat.    The
time value given for CBIRTH should be set to a time later in the
simulation after the forming process is well underway. 
CDEATH 
Death time for adaptive fusion. 
LCLVL 
Load  curve  ID  of  a  curve  that  defines  the  maximum  refinement
level as a function of time 
CNLA 
Limit angle for corner nodes.  See Remark 7. 
MMM2D 
ADPERR 
If non-zero, common  boundaries of all adapted materials will be
merged.  Only for 2D r-adaptivity 
3-digit  number,  as  “𝑋𝑌𝑌”,  where  “𝑋”  and  “𝑌𝑌”  define  the 
options  for  the  recovery  techniques  and  the  error  estimators,
VARIABLE   
DESCRIPTION
respectively,  
For 𝑋: 
EQ.0: superconvergent patch recovery (SPR) (default);  
EQ.1: the least square fit of the stress to the nodes (Global L2); 
EQ.2: error density SPR, as Δ𝑒 ̃ = Δ𝑒/Areaelement;  
EQ.3: self-weighted SPR, as Δ𝑒 ̊ = √Δ𝑒 × 𝑒 
For 𝑌𝑌: 
EQ.00:  energy norm (default) 
EQ.01:  Cauchy 𝜎𝑥 
EQ.02:  𝜎𝑦 
EQ.03:  𝜎𝑧 
EQ.04:  𝜏𝑥𝑦 
EQ.05:  𝜏𝑦𝑧 
EQ.06:  𝜏𝑧𝑥 
EQ.07:  effective plastic strain, 𝜀ep 
EQ.08:  pressure 
EQ.09:  von Mises 
EQ.10:  principal deviator stress s11 
EQ.11:  𝑆22 
EQ.12:  𝑆33 
EQ.13:  Tresca 
EQ.14:  principal stress 𝜎11 
EQ.15:  𝜎22 
EQ.16:  𝜎33 
EQ.20:  user  subroutine  “uadpval”  to  extract  the  numerical 
solutions  for  recovery,  and  “uadpnorm”  to  provide  an 
error estimator. 
D3TRACE 
Flag  that  is  either  0  or  1.    If  set  to  1  then  a  d3plot  state  will  be 
output just before and after an adaptive step even though it may
not be requested.  The reason for wanting to do this is to allow the
LS-PrePost  particle  trace  algorithm  to  work  in  the  case  of
VARIABLE   
DESCRIPTION
adaptivity. 
IFSAND 
Set this flag to “1” for forming of sandwiched parts with adaptive 
blank  mesh,  see  Remarks.    Currently  the  adaptivity  is  limited  to 
only one layer of solid element, and applies to ADPOPT = 1 and 2 
only.  
Remarks about 3D adaptivity: 
1.  Restarting.    The d3dump  and  runrsf  files  contain  all  information  necessary  to 
restart an adaptive run.  This did not work in version 936 of LS-DYNA. 
2.  Related  Field  in  *PART.    In  order  for  this  control  card  to  work,  the  flag 
ADPOPT=1 must be set in the *PART definition.  Otherwise, adaptivity will not 
function. 
3.  Contact  Types  and  Options.    In  order  for  adaptivity  to  work  optimally,  the 
parameter  SNLOG=1,  must  be  set  on  Optional  Control  Card  B  in  the  *CON-
TACT  Section.    On  disjoint  tooling  meshes  the  contact  option  *CONTACT_-
FORMING_… is recommended. 
4.  Root ID (RID) File.  A file named “adapt.rid” is left on disk after the adaptive 
run is completed.  This file contains the root ID of all elements that are created 
during the calculation, and it does not need to be kept if it is not used in post-
processing. 
5.  Note  About  IADPN90  Field.    For  all  metal  forming  simulation,  IADPN90 
should be set to -1. 
6.  Contact and ADPENE.  In three dimensions when ADPENE>0 it is presumed 
that the solid part to be adapted is on the slave side of a contact, and the “tool-
ing”,  consisting  of  a  shell  surface,  is  on  the  master  side  of  that  same  contact.  
ADPENE>0  represents  a  distance  from  the  tooling  surface  within  which  the 
adapted mesh refinement of the slave part is influenced by the radius of curva-
ture  of  the  tooling  surface.    This  feature  is  currently  unavailable  in  SMP  and 
SOFT=2 in *CONTACT. 
Remarks about 2D r-adaptivity: 
7.  CNLA  Field.    In  two  dimensions  𝑟-adaptive  remeshing,  the  generated  new 
mesh should have a node at each corner so that corners are not smoothed.  By 
default,  the  mesher  will  assume  a  corner  wherever  the  interior  angel  between 
adjacent edges is less than 110 degrees.  Setting CNLA larger than 110 enables
angles larger than 110 to be corners.  Care should be taken to avoid an unneces-
sarily  large  value  of  CNLA  as  this  may  prevent  the  mesher  from  generating 
smooth meshes. 
Remarks about mesh adaptivity for sandwiched parts (IFSAND): 
8.  Sandwiched parts (also called laminates) consist layers of solid elements (core) 
sandwiched  by  one  layer  of  shell  elements  each  on  top  and  bottom  surface  of 
the solid elements, as shown in Figure 12-3.  Common nodes are used for solid 
and  shell  interface.    Currently  mesh  adaptivity  is  limited  to  only  one  layer  of 
solid element with mesh refinements in-plane on both solids and shells. 
Note  sandwiched  parts  can  be  trimmed  by  setting  ITYP = 1  in  keyword 
keyword 
*CONTROL_FORMING_TRIMMING 
*DEFINE_CURVE_TRIM.    Trimming  of  sandwiched  parts  allows  for  multiple 
layers of solids. 
with 
and 
In a typical forming set up, the following cards need to be changed to activate 
the sandwiched part mesh adaptivity: 
*CONTROL_ADAPTIVE 
$# adpfreq    adptol    adpopt    maxlvl    tbirth    tdeath     lcadp    ioflag 
   &adpfq 4.0000E+00         1         4     0.0001.0000E+20         0         0 
$# adpsize    adpass    ireflg    adpene     adpth    memory    orient     maxel 
   0.90000         1            10.00000     0.000         0         0         0 
$# ladpn90    ladpgh    ncfred    ladpcl    adpctl    cbirth    cdeath     lclvl 
        -1         0         0         1     0.000     0.0001.0000E+20         0 
$                                                                         IFSAND 
                                                                               1 
*PART 
Mid-core layer of solid elements 
$      PID     SECID       MID     EOSID      HGID      GRAV    ADPOPT      TMID 
         1         1         1                                       1 
Top layer of shell elements 
       100       100         1                                       1 
Bottom layer of shell elements 
       101       100         1                                       1 
Note IFSAND in *CONTROL_ADAPTIVE is set to “1” to activate the sandwich 
part adaptivity; ADPOPT under *PART are all set to “1” to activate the adaptivity. 
Revision Information: 
9. 
IFSAND  is  available  starting  in  Rev  104365  in  both  SMP  and  MPP  versions.  
Later revisions may include improvements.
layer  of 
Top 
shell elements
Only 1 layer of 3-D 
solid  elements  are 
allowed
Bottom layer of shell elements
Figure 12-3.  Mesh adaptivity of sandwiched parts (IFSAND).
*CONTROL_ADAPTIVE_CURVE 
Purpose:    To  refine  the  element  mesh  along  a  curve  during  or  prior  to  sheet  metal 
forming  simulation.    All  curves  defined  by  the  keyword  *DEFINE_CURVE_TRIM  are 
used  in  the  refinement.    This  option  provides  additional  refinement  to  that  created  by 
*CONTROL_ADAPTIVE.    Additionally,  pre-mesh  refinement  along  a  curve  with 
specific distance/range on both sides of the curve can be modeled when this keyword is 
used  together  with  *DEFINE_CURVE_TRIM_3D  (by  activating  the  variable  TCTOL).  
Lastly,  the  keyword  can  be  used  to  refine  mesh  along  a  curve  during  trimming  when 
used together with the keyword *ELEMENT_TRIM.  This feature only applies to shell 
elements. 
  Card 1 
1 
2 
Variable 
IDSET 
ITYPE 
Type 
I 
I 
3 
N 
I 
4 
5 
6 
7 
8 
SMIN 
ITRIOPT 
F 
I 
  VARIABLE   
DESCRIPTION
IDSET 
ITYPE 
Set ID 
Set type: 
EQ.1: IDSET is shell set ID. 
EQ.2: IDSET is part set ID. 
N 
Refinement option: 
EQ.1: Refine  until  there  are  no  adaptive  constraints  remaining
in  the  element  mesh  around  the  curve,  subjected  to  the 
maximum refinement level of 5. 
GT.1: Refine no more than N levels. 
SMIN 
If the element dimension is smaller than this value, do not refine. 
ITRIOPT 
Option to refine an enclosed area of a trim curve. 
EQ.0: Refine the elements along the trim curve. 
EQ.1: Refine the elements along the trim curve and enclosed by
the trim curve.
Adaptive mesh refinement along a curve during a simulation: 
In Figure 12-4, an example is shown to illustrate the mesh adaptivity along an enclosed 
curve.  Since the mesh refinement is controlled by the refinement level “N” and smallest 
element  size  “SMIN”,  care  should  be  taken  so  not  too  many  elements  are  generated 
during the run. 
A partial input example is listed below, where mesh will be refined by four levels, or to 
no  smaller  than  0.3mm  element  edge  length, along  both  sides  of  the  curve  defined  by 
IGES format file “adpcurves.iges”. 
*INCLUDE 
drawn.dynain 
*DEFINE_CURVE_TRIM_3D 
$     TCID    TCTYPE      TFLG      TDIR     TCTOL 
         1         2 
adpcurves.iges                                                         
*CONTROL_ADAPTIVE_CURVE 
$    IDSET     ITYPE         N      SMIN 
         1         2         4       0.3 
Since this method tends to create too many elements during refinement, the following 
feature was added to address the issue. 
Adaptive mesh refinement along a curve in the beginning of a simulation: 
When TCTOL is defined under the keyword *DEFINE_CURVE_TRIM_3D, it is used as 
a  distance  definition,  and  together  with  *CONTROL_ADAPTIVE_CURVE,  the  mesh 
will be refined in the beginning of a (flanging, etc.) simulation, along both sides of the 
defined curve, limited within the distance specified, as shown in Figures 12-5 and 12-6.  
In addition, this feature works with the option 3D only.  It is noted that the curve needs 
to  be  sufficient  close  to  the  part,  and  this  can  be  accomplished  in  LS-PrePost4.0  under 
GeoTol/Project/Closest  Proj/Project  to  Element/By  Part.    Furthermore,  since  the  curve  is 
often  made  from  some  feature  lines  of  forming  tools,  it  is  important  the  curve  is  re-
positioned  closer  to  the  blank,  or  better  yet, is  projected  onto  the  blank;  otherwise  the 
refinement will not take place.  A partial input example is listed below, where mesh will 
be refined within a range of 4.0mm,  formed by 2.0mm distance (TCTOL = 2.0) of both 
sides of the curve, defined by file “adpcurves.iges”.  The maximum refine level is 4 and 
minimum element size allowed is 0.3mm.  
*INCLUDE 
drawn.dynain 
*DEFINE_CURVE_TRIM_3D 
$     TCID    TCTYPE      TFLG      TDIR     TCTOL      
         1         2         0         0     2.000      
adpcurves.iges                                                         
*CONTROL_ADAPTIVE_CURVE 
$    IDSET     ITYPE         N      SMIN 
         1         2         4       0.3 
Mesh refinement along a curve is very useful during line die simulation.  For example, 
in a flanging simulation, a trimmed blank, where it is mostly flat in the flanging break
line in draw die, can be refined using a curve generated from the trim post radius.  In 
LS-PrePost 4.0, the curve can be generated using Curve/Spline/From Mesh/By Edge, check 
Prop,  and  defining  a  large Ang  to  create  a  continuous  curve  along  element  edge.    This 
curve can then be projected onto the blank mesh using GeoTol/Project feature, to be used 
as  the  curve  file  “adpcurves.iges”  here.    The  mesh  pre-refinement  along  curves  are 
implemented  in  ‘flanging’  process  starting  in  LS-PrePost4.0  eZSetup  for  metal  forming 
application.    In  LS-PrePost4.3  eZSetup,  improvements  are  made  so  adaptive  mesh 
refinement along a curve can be made without the need to define any tools. 
In  Figures  12-7,  12-8,  12-9,  12-10and  12-11,  mesh  pre-refinement  along  a  curve  is 
demonstrated  on  the  fender  outer  case.    The  effect  of  different  TCTOL  values  on  the 
mesh refinement is obvious. 
The keyword *INCLUDE_TRIM is recommended to be used at all times to include the 
dynain file from a previous simulation, except in case where to-be-adapted sheet blank 
has  no  stress  and  strain  information  (no  *INITIAL_STRESS_SHELL,  and  *INITIAL_-
STRAIN_SHELL  cards  present  in  the  sheet  blank  keyword  or  dynain  file),  then  the 
keyword *INCLUDE must be used. 
Adaptive mesh refinement along a curve during trimming: 
When this keyword *ELEMENT_TRIM is present, this keyword is used to refine meshes 
during a trimming simulation.  Coarse meshes along the trim curve can be refined prior 
to trimming, leaving a more detailed and distinctive trim edge.  A partial example input 
deck is shown below: 
*INCLUDE_TRIM 
drawn.dynain 
*ELEMENT_TRIM 
         1 
*DEFINE_CURVE_TRIM_NEW 
$#    TCID    TCTYPE      TFLG      TDIR     TCTOL      TOLN    NSEED1    NSEED2 
         1         2                   0     0.250         1 
doubletrim.iges 
*DEFINE_TRIM_SEED_POINT_COORDINATES 
$    NSEED        X1        Y1        Z1        X2        Y2        Z2 
         1  -184.565    84.755 
*CONTROL_ADAPTIVE_CURVE 
$#   IDSET     ITYPE         N      SMIN   ITRIOPT 
         1         2         3       3.0         0 
*CONTROL_CHECK_SHELL 
$#    PSID    IFAUTO    CONVEX      ADPT     ARATIO    ANGLE      SMIN 
         1         1         1         1       0.25    150.0      0.18 
Where  the  keyword  *ELEMENT_TRIM  is  used  to  define  a  deformable  part  set  to  be 
trimmed.  The keyword *DEFINE_CURVE_TRIM_NEW is used to define the trim curve 
and 
keyword 
*DEFINE_TRIM_SEED_POINT_COORDINATES 
is  used  to  define  a  seed  point 
coordinate  located  on  the  portion  that  remains  after  trimming.    The  keyword 
tolerance, 
along 
type, 
with 
trim 
The 
etc.
*CONTROL_ADAPTIVE_CURVE is used to define the adaptive mesh refinement level 
and  minimum  element  size  along 
the  keyword 
the 
*CONTROL_CHECK_SHELL  is  used  to  repair  and  fix  trimmed  elements  so  they  are 
suitable  for  next  stage  simulation.    More  details  can  be  found  in  each  of  the 
corresponding keyword manual section. 
trim  curve. 
  Finally,
Figure 12-4.  Mesh refinement along a curve 
Curves defining 
adaptive mesh location
Formed blank
Figure 12-5.  Curves can be discontinuous and in one IGES file. 
Figure 12-6.  Define variable TCTOL to limit the mesh adaptivity area. 
TCTOL
Trim panel 
Curve defining pre-adaptive area 
Flanging area mating 
with hood inner 
Figure  12-7.    A  complex  mesh  refinement  example  (NUMISHEET2002
Fender). 
Curve defining center 
of adaptive band
Figure 12-8.  Original mesh with target curves defined.
Figure 12-9.  Mesh refinement with TCTOL = 0.5. 
0.5 mm
1.0 mm
Figure 12-10.  Mesh refinement with TCTOL = 1.0.
2.0 mm
Figure 12-11.  Mesh refinement with TCTOL = 2.0.
*CONTROL_ALE 
Purpose:    Set  global  control  parameters  for  the  Arbitrary  Lagrangian-Eulerian  (ALE) 
and Eulerian calculations.  This command is required when solid element formulation 
5, 6, 7, 11, or 12 is used.  Parallel processing using SMP is not recommended when using 
these  element  formulations,  rather  it  is  better  to  use  MPP  for  good  parallel  processing 
performance. 
  See  *CONTROL_MPP_DECOMPOSITION_DISTRIBUTE_ALE_ELE-
MENTS. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DCT 
NADV 
METH 
AFAC 
BFAC 
CFAC 
DFAC 
EFAC 
Type 
Default 
I 
1 
  Card 2 
1 
I 
0 
2 
I 
1 
3 
F 
0 
4 
F 
0 
5 
F 
0 
6 
F 
0 
7 
F 
0 
8 
Variable 
START 
END 
AAFAC 
VFACT 
PRIT 
EBC 
PREF 
NSIDEBC 
Type 
Default 
F 
0 
F 
1020 
F 
1 
F 
F 
10-6 
0.0 
I 
0 
F 
I 
0.0 
none 
This card is optional. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NCPL 
NBKT 
IMASCL 
CHECKR 
BEAMIN  MMGPREF  PDIFMX  DTMUFAC
Type 
Default 
I 
1 
I 
50 
I 
0 
F 
F 
0.0 
0.0 
I 
0 
F 
F 
0.0 
0.0
*CONTROL 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  OPTIMPP 
Type 
Default 
I 
0 
  VARIABLE   
DCT 
DESCRIPTION
Flag to invoke alternate advection logic.  Formerly flag to control
default continuum treatment: 
NE.-1:  Use default advection logic. 
EQ.-1:  Use  alternate  advection  logic;  generally  recommended,
especially for simulation of explosives . 
NADV 
Number of cycles between advections (almost always set to 1). 
METH 
Advection method: 
EQ.1:  Donor  cell  with  Half  Index  Shift  (HIS),  first  order
accurate. 
EQ.2:  Van Leer with HIS, second order accurate. 
EQ.-2:  Van Leer with HIS: 
Additionally,the  monotonicity 
condition  is  relaxed  during  advection  process  to  better
preserve 
*MAT_HIGH_EXPLOSIVE_BURN  material 
interfaces.   
EQ.3:  Donor  cell  with  HIS  modified  to  conserve  total  energy
over  each  advection  step,  in  contrast  to  METH = 1 
which conserving internal energy . 
AFAC 
ALE smoothing weight factor - Simple average: 
EQ.-1:  turn smoothing off: 
. 
BFAC 
CFAC 
DFAC 
ALE smoothing weight factor – Volume weighting 
ALE smoothing weight factor – Isoparametric 
ALE smoothing weight factor – Equipotential
VARIABLE   
DESCRIPTION
EFAC 
ALE smoothing weight factor – Equilibrium 
START 
END 
Start  time  for  ALE  smoothing  or  start  time  for  ALE  advection  if
smoothing is not used. 
End  time  for  ALE  smoothing  or  end  time  for  ALE  advection  if
smoothing is not used. 
AAFAC 
ALE advection factor (donor cell options, default = 1.0) 
VFACT 
Volume  fraction  limit  for  stresses  in  single  material  and  void
formulation.  All stresses are set to zero for elements with lower
volume fraction than VFACT. 
EQ.0.0: set to default 10−6   
PRIT 
A flag to turn on or off the pressure equilibrium iteration option
for multi-material elements . 
EQ.0: Off (default) 
EQ.1: On 
EBC 
Automatic Eulerian boundary condition . 
EQ.0: Off 
EQ.1: On with stick condition 
EQ.2: On with slip condition 
PREF 
NSIDEBC 
NCPL 
Reference  pressure  to  compute  the  internal  forces.    . 
A  node  set  ID  (NSID)  which  is  to  be  excluded  from  the  EBC 
constraint. 
Number  of  Lagrangian  cycles  between  coupling  calculations.
This is typically done every cycle; therefore, its default is 1.  This
is on optional card 3.
NBKT 
IMASCL 
*CONTROL 
DESCRIPTION
Number  of  Lagrangian  cycles  between  global  bucket-sort 
searches to locate the position of the Lagrangian structure (mesh)
relative to the ALE fluid (mesh).  Default is 50.  This is on optional
card 3.  
LT.0:  |NBKT| is a *DEFINE_CURVE ID defining a table: time 
vs NBKT as defined above 
EQ.0: (Default) NBKT = 50: 
If the mesh is moving, NBKT is 
adapted for the buckets to follow the mesh more closely 
GT.0:  NBKT remains constant. 
A  flag  for  turning  ON/OFF  mass  scaling  for  ALE  parts.    The
global  mass  scaling  control  (parameter  DT2MS  under  *CON-
TROL_TIMESTEP card) must be ON.  If the run dt is lower than
the mass scaling dt, then IMASCL has the following effects: 
EQ.0: (Default)  No  mass  scaling  for  ALE  parts.    Print  out 
maximum 20 warnings. 
EQ.1: No mass scaling for ALE parts.  Stop the run. 
EQ.2: Do  mass  scaling  for  ALE  parts  (the  result  may  not  be
correct due to this scaling). 
EQ.3: No mass scaling for ALE parts.  Timestep is taken as the 
minimum of the ALE timestep and DT2MS.  
CHECKR 
BEAMIN 
A parameter for reducing or eliminating an ALE pressure locking
pattern.  It may range from 0.01 to 0.1 . 
Flag  to  align  the  dynamics  of  plain  strain  and  axisymmetric 
beams in  2D FSI ALE models to their shell counterparts in 3D FSI
ALE models: 
EQ.0.0: Off (default) 
EQ.1.0: On
MMGPREF 
*CONTROL_ALE 
DESCRIPTION
MMGPREF selects the method that is used to include a reference
pressure  in  a  calculation  involving  ALE  multi-material  groups 
. 
LT.0:  |MMGPREF|  is  the  id  of  a  table  defined  by  *DEFINE_-
CURVE where the abscissas are the multi-material group 
ids and the ordinates are the reference pressures. 
If a multi-material group is not in the table, its reference 
pressure is default to PREF. 
For  situations  in  which  the  reference  pressures  are  time
dependent  *DEFINE_TABLE  should  be  used  instead  of 
*DEFINE_CURVE.    The  table  should  consist  of  a  set  of
curves indexed by group ID that encode reference pres-
sure  as  a  function  of  time.    If  𝑛  groups  need  reference 
pressure  histories,  *DEFINE_TABLE  will  have  𝑛  lines 
followed by 𝑛 corresponding *DEFINE_CURVE. 
EQ.0: Off (default). 
EQ.1: Obsolete:  Use MMGPREF < 0 instead 
EQ.2: Obsolete:  Use MMGPREF < 0 instead 
PDIFMX 
Maximum  of  pressure  difference  between  neighboring  ALE
elements under which the stresses are zeroed out: 
EQ.0: Off (default) 
GT.0:  On 
DTMUFAC 
Scale  a  time  step  called  DTMU  that  depends  on  the  dynamic
viscosity  𝜇,  the  initial  density  𝜌,  and  an  element  characteristic 
length ℓ: 
DTMU =
𝜌ℓ2
2𝜇
DTMU is emitted by the element to the solver as an element time
step, thereby making DTMU an upper bound on the global time 
step. 
EQ.0: Off (default) 
GT.0:  On
Optimize  the  MPP  communications  in  the  penalty  coupling
(*CONSTRAINED_LAGRANGE_IN_SOLID,  CTYPE = 4)  and 
group ALE parts together for the element processing.  
EQ.0: Off (default) 
EQ.1: On 
*CONTROL_ALE 
  VARIABLE   
OPTIMPP 
Remarks: 
1.  The PRIT Field.  Most of the fast transient applications do not need this feature.  
It could be used in specific slow dynamic problems for which material constitu-
tive laws with very different compressibility are linear and the stresses in multi-
material elements require to be balanced. 
2.  The  EBC  Field.    This  option,  used  for  EULER  formulations.    It  automatically 
defines  velocity  boundary  condition  constraints  for  the  user.    The  constraints, 
once  defined,  are  applied  to  all  nodes  on  free  surfaces  of  an  Eulerian  domain.  
For problems where the normal velocity of the material at the boundary is zero 
such as injection molding problems, the automatic boundary condition parame-
ter is set to 2.  This will play the same role as the nodal single point constraint.  
For  EBC = 1,  the  material  velocity  of  all  free  surface  nodes  of  an  Eulerian  do-
main is set to zero. 
3.  The PREF Field.  The reference pressure PREF is subtracted from the stresses 
before  computing  the  internal  forces.    Thus  PREF  is  equivalent  to  applying  a 
*LOAD_SEGMENT  card  to  balance  the  internal  pressure  along  the  ALE  mesh 
boundaries.    PREF  is  applied  to  all  the  materials  in  the  ALE  mesh.    So,  before 
the subtraction for MMGPREF > 0, PREF is added to the stresses of some mate-
rials. 
On another hand, MMGPREF < 0 subtracts a reference pressure depending on 
ALE MMG ID.  The shift of the stresses by PREF is not necessary (and so it can 
not be seen in the LS-PrePost fringe of the pressures).  For example, if a model 
has 3 ALE groups: air with an initial pressure of 1.0 bar, an explosive material, 
and  water,  the  reference  pressure  of  the  first  group  would  be  1.0  bar  whereas 
the  other  groups  would  have  none.    In  that  case,  PREF = 0.0  bar  and 
MMGPREF = -LCID where LCID is the id of the following table: 
*DEFINE_CURVE 
lcid 
1,1.0 
2,0.0 
3,0.0
4.  CHECKR Field for One Point Integration.  Due to one point integration, ALE 
elements may experience a spatial instability in the pressure field referred to as 
checker boarding.  CHECKR is a scale for diffusive flux calculation to alleviate 
this problem. 
5.  METH=3  for  Conserving  Total  Energy.    Generally,  it  is  not  possible  to 
conserve both momentum and kinetic energy (KE) at the same time.  Typically, 
internal energy (IE) is conserved and KE may not be.  This may result in some 
KE  loss  (hence,  total  energy  loss).    For  many  analyses  this  is  tolerable,  but  for 
airbag  application,  this  may  lead  to  the  reduction  of  the  inflating  potential  of 
the inflator gas.  METH=3 tries to eliminate this loss in KE over the advection 
step  by  storing  any  loss  KE  under  IE,  thus  conserving  total  energy  of  the  sys-
tem. 
6.  Smoothing Factors.    All  the  smoothing  factors  (AFAC,  BFAC,  CFAC,  DFAC, 
EFAC) are generally most applicable to ELFORM = 5 (single material ALE for-
mulation).  The ALE smoothing feature is not supported by MPP versions. 
7.  First Pass Recommendations.  Although this card has many parameters, only 
a  few  are  required  definitions.    Typically,  one  can  try  setting  NADV=1, 
METH=1,  AFAC=-1  and  the  rest  as  “0”  as  a  starting  point.    Sometimes  when 
needed, PREF should be defined.  This is adequate for most cases.  Sometimes it 
may  be  appropriate  to  fine-tune  the  model  by  changing  METH  to  2  or  3  de-
pending on the physics. 
8.  Pressure  Checker  Boarding.    Because  the  internal  forces  are  located  at  the 
nodes, while the pressure is stored at the element center, sometimes a "checker-
board pattern" arises in the pressure distribution.  It is a kind of locking effect 
that normally occurs only in problems having very small volumetric strains, i.e., 
at small pressures.  “CHECKR” is designed for alleviating this problem. 
9.  The  DCT  Field.    Starting  with  the  R5  the  DCT  field  can  be  used  to  invoke  an 
alternate advection scheme.  DCT=-1 is recommended over the default scheme, 
especially for simulating explosives and includes the following major changes: 
a)  Relaxes  an  artificial  limit  on  the  expansion  ratio  limit.    The  default  limit 
improves  stability  in  some  situations  but  can  overestimate  the  explosive 
impulse.  
b)  Corrects  redundant  out-flux  of  material  at  corner  elements.    The  redun-
dancy can lead to negative volume. 
c)  Removes  several  artificial  constraints  in  the  advection  which  were  origi-
nally implemented to assist in stability but are no longer needed.
10.  METH = -2.  The METH = -2 advection type is the same as METH = 2 with only 
one  exception.    It  employs  a  looser  constraint  on  monotonicity  requirement 
during  ALE  advection.    When  METH = 2,  for  each  advection  process  along 
three  directions  (front/back,  top/bottom,  left/right),  the  maximum/minimum 
values for advected history variables in the three elements along that direction 
are capped.  METH = -2 relaxed the monotonicity condition so that the advec-
ted value is capped at the maximum/minimum value in the element itself and 
its neighboring 26 elements.  This option, in certain conditions, can better pre-
serve  the  material  interface  for  materials  defined  with  *MAT_HIGH_EXPLO-
SIVE_BURN.
*CONTROL_BULK_VISCOSITY 
Purpose:  Reset the default values of the bulk viscosity coefficients globally.  This may 
be advisable for shock wave propagation and some materials.  Bulk viscosity is used to 
treat  shock  waves.    A  viscous  term  q  is  added  to  the  pressure  to  smear  the  shock 
discontinuities  into  rapidly  varying  but  continuous  transition  regions.    With  this 
method the solution is unperturbed away from a shock, the Hugoniot jump conditions 
remain valid across the shock transition, and shocks are treated automatically.  
  Card 1 
Variable 
1 
Q1 
Type 
F 
2 
Q2 
F 
Default 
1.5 
.06 
3 
4 
5 
6 
7 
8 
TYPE 
BTYPE 
I 
1 
I 
0 
  VARIABLE   
DESCRIPTION
Q1 
Q2 
Default quadratic viscosity coefficient. 
Default linear viscosity coefficient. 
TYPE 
Default bulk viscosity type, IBQ (Default = 1) 
EQ.-2:  standard  (also  types  2,  4,  10,  16,  and  17).    With  this
option the internal energy dissipated by the viscosity in
the  shell  elements  is  computed  and  included  in  the
overall energy balance. 
EQ.-1:  standard (also types 2, 4, 10, 16, and 17 shell elements).
The  internal  energy  is  not  computed  in  the  shell  ele-
ments. 
EQ.+1:  standard:  Solid  elements  only  and  internal  energy  is
always  computed  and  included  in  the  overall  energy
balance. 
EQ.+2:  Richards-Wilkins:  Two-dimensional  plane  strain  and 
axisymmetric  solid  elements  only.    Internal  energy  is 
always  computed  and  included  in  the  overall  energy
balance.
VARIABLE   
DESCRIPTION
BTYPE 
Beam bulk viscosity type (Default = 0) 
EQ.0:  The bulk viscosity is turned off for beams. 
EQ.1:  The bulk viscosity is turned on for beam types 1 and 11.
The  energy  contribution  is  not  included  in  the  overall
energy balance. 
EQ.2:  The  bulk  viscosity  is  turned  on  for  beam  type  1  and  11.
The energy contribution is included in the overall energy
balance. 
Remarks: 
The bulk viscosity creates an additional additive pressure term given by: 
𝑞 = {
𝜌𝑙(𝑄1𝑙𝜀̇𝑘𝑘
2 − 𝑄2𝑎𝜀̇𝑘𝑘)
𝜀̇𝑘𝑘 < 0
𝜀̇𝑘𝑘 ≥ 0
where  𝑄1  and  𝑄2  are  dimensionless  input  constants  which  default  to  1.5  and  .06, 
respectively, and 𝑙 is a characteristic length given as the square root of the area in two 
dimensions and as the cube root of the volume in three, 𝑎 is the local sound speed, 𝑄1 
defaults to 1.5 and 𝑄2 defaults to .06.  See Chapter 21 in the LS-DYNA Theory Manual 
for more details. 
The  Richards-Wilkins,  see  [Richards    1965,  Wilkins  1976],  bulk  viscosity  considers  the 
directional  properties  of  the  shock  wave.    This  has  the  effect  of    turning  off  the  bulk 
viscosity in converging geometries minimizing the effects of “q-heating”.  The standard 
option  is  active  whenever  the  volumetric  strain  rate  is  undergoing  compression  even 
though no shock waves are present.
Purpose:  Check for various problems in the mesh. 
*CONTROL_CHECK_SHELL 
Part cards.  Include one card for each part or part set to be checked.  The next keyword 
(“*”) card terminates this input. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PSID 
IFAUTO 
CONVEX 
ADPT 
ARATIO 
ANGLE 
SMIN 
Type 
Default 
I 
0 
I 
0 
I 
1 
I 
1 
F 
F 
F 
0.25 
150.0 
0.0 
  VARIABLE   
DESCRIPTION
PSID 
Part or part set ID to be checked: 
EQ.0: do not check 
GT.0:  part ID 
LT.0:  part set ID 
IFAUTO 
Flag to automatically correct bad elements: 
EQ.0: write warning message only  
EQ.1: fix bad element, write message 
CONVEX 
Check element convexity (internal angles less than 180 degrees) 
EQ.0: do not check 
EQ.1: check 
ADPT 
Check adaptive constraints 
EQ.0: do not check 
EQ.1: check 
ARATIO 
Minimum  allowable  aspect  ratio.    Elements  which  do  not  meet
minimum  aspect  ratio  test  will  be  treated  according  to  IFAUTO
above. 
ANGLE 
Maximum allowable internal angle.  Elements which fail this test
will be treated according to IFAUTO above.
DESCRIPTION
Minimum  element  size.    Elements  which  fail  this  test  will  be
treated according to IFAUTO above. 
  VARIABLE   
SMIN 
Remarks: 
1.  For  the  SHELL  option,  shell  element  integrity  checks  which  have  been 
identified  as  important  in  metal  forming  applications  are  performed.    These 
checks  can  improve  springback  convergence  and  accuracy.    This  option  will 
repair bad elements created, for example, during trimming operations. 
2. 
3. 
If  the  convexity  test  is  activated,  all  failed  elements  will  be  fixed  regardless  of 
IFAUTO. 
In addition to illegal constraint definitions (slave which is also a master), checks 
are performed for mesh connectivities which have been found to cause conver-
gence trouble in implicit springback applications. 
4.  Variable SMIN should be set to 1/4 to 1/3 of smallest pre-trim element length.  
In an example below, smallest element length pre-trim is 0.6mm, which makes 
SMIN to be 0.18: 
*CONTROL_CHECK_SHELL 
1,1,1,1,0.25,150.0,0.18 
$ smin=(0.25~0.3)*smallest pre-trim element length, which is ~0.6 mm. 
5.  Shell checking is done during the input phase (in sprinback input deck) in LS-
DYNA R5 Revision 63063 and prior releases.  After the Revision, it is done after 
trimming  is  completed.    Therefore  the  keyword  should  be  included  in  a  trim-
ming input deck.
*CONTROL_COARSEN 
Purpose:    Adaptively  de-refine  (coarsen)  a  shell  mesh  by  selectively  merging  four 
adjacent elements into one.  Adaptive constraints are added and removed as necessary. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ICOARSE 
ANGLE 
NSEED 
PSID 
SMAX 
Type 
Default 
  Card 2 
Variable 
Type 
Default 
I 
0 
1 
N1 
I 
0 
F 
none 
2 
N2 
I 
0 
I 
0 
3 
N3 
I 
0 
I 
0 
4 
N4 
I 
0 
F 
0 
5 
N5 
I 
0 
  VARIABLE   
DESCRIPTION
ICOARSE 
Coarsening flag: 
EQ.0: do not coarsen (default) 
6 
N6 
I 
0 
7 
N7 
I 
0 
8 
N8 
I 
0 
EQ.1: coarsen  mesh  at  beginning  of  simulation  for  forming
model 
EQ.2: coarsen mesh at beginning of simulation for crash model
ANGLE 
Allowable angle change between neighboring elements.  Adjacent
elements  which  are  flat  to  within  ANGLE  degrees  are  merged.
(Suggested starting value = 8.0 degrees) 
NSEED 
Number of seed nodes (optional).   
EQ.0: use only automatic searching. 
GT.0: the number of seed nodes with which to supplement the
search  algorithm.    See  Remark  2.    NSEED  must  be  an
integer less than or equal to 8.
VARIABLE   
DESCRIPTION
PSID 
SMAX 
Part  set  ID.    All  the  parts  defined  in  this  set  will  be  prevented
from been coarsened. 
Maximum  element  size.    For  ICOARSE = 2,  no  elements  larger 
than this size will be created. 
N1, …, N8 
Optional  list  of  seed  node  IDs  for  extra  searching.    If  no  seed
nodes are specified, leave card 2 blank. 
Remarks: 
1.  Coarsening  is  performed  at  the  start  of  a  simulation.    The  first  plot  state 
represents  the  coarsened  mesh.    By  setting  the  termination  time  to  zero  and 
including  the  keyword  *INTERFACE_SPRINGBACK_LSDYNA  a  keyword 
input deck can be generated containing the coarsened mesh. 
2.  By  default,  an  automatic  search  is  performed  to  identify  elements  for  coarsen-
ing.  In some meshes, isolated regions of refinement may be overlooked.  Seed 
nodes  can  be  identified  in  these  regions  to  assist  the  automatic  search.    Seed 
nodes identify the central node of a four-element group which is coarsened into 
a single element if the angle criterion is satisfied. 
3.  The keyword *DEFINE_BOX_COARSEN can be used to indicate regions of the 
mesh which are protected from coarsening.
*CONTROL_CONTACT 
Purpose:  Change defaults for computation with contact surfaces. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SLSFAC  RWPNAL 
ISLCHK 
SHLTHK 
PENOPT 
THKCHG 
ORIEN 
ENMASS 
Type 
F 
F 
Default 
.1 
none 
Remarks 
  Card 2 
1 
2 
I 
1 
3 
3 
I 
0 
I 
1 
I 
0 
I 
1 
I 
0 
4 
5 
6 
7 
8 
Variable 
USRSTR  USRFRC 
NSBCS 
INTERM 
XPENE 
SSTHK 
ECDT 
TIEDPRJ 
Type 
Default 
I 
0 
I 
0 
I 
10-100
I 
0 
F 
4.0 
I 
0 
I 
0 
I 
0 
Remaining cards are optional.† 
The optional cards apply only to the following contact types: 
*SINGLE_SURFACE 
*AUTOMATIC_GENERAL 
*AUTOMATIC_SINGLE_SURFACE 
*AUTOMATIC_NODES_TO_… 
*AUTOMATIC_SURFACE_… 
*AUTOMATIC_ONE_WAY_… 
*ERODING_SINGLE_SURFACE.
The  friction  coefficients  SFRIC,  DFRIC,  EDC,  and  VFC  are  active  only  when  *PART_-
CONTACT  is  invoked  with  FS = -1  in  *CONTACT,  and  the  corresponding  frictional 
coefficients  in  *PART_CONTACT  are  set  to  zero.    This  keyword’s  TH,  TH_SF,  and 
PEN_SF  override  the  corresponding  parameters  in  *CONTACT,  but  will  not  override 
corresponding nonzero parameters in *PART_CONTACT. 
  Card 3 
1 
2 
3 
4 
Variable 
SFRIC 
DFRIC 
EDC 
VFC 
Type 
F 
F 
F 
F 
5 
TH 
F 
6 
7 
8 
TH_SF 
PEN_SF 
PTSCL 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
1.0 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IGNORE 
FRCENG  SKIPRWG OUTSEG  SPOTSTP SPOTDEL  SPOTHIN 
Type 
Default 
I 
0 
  Card 5 
1 
I 
0 
2 
I 
0 
3 
I 
0 
4 
I 
0 
5 
I 
F 
0 
inactive 
6 
7 
8 
Variable 
ISYM 
NSEROD  RWGAPS  RWGDTH
RWKSF 
ICOV 
SWRADF 
ITHOFF 
Type 
Default 
I 
0 
I 
0 
I 
0 
F 
0. 
F 
1.0 
I 
0 
F 
0. 
I
Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SHLEDG 
PSTIFF 
ITHCNT 
TDCNOF 
FTALL 
SHLTRW 
IGACTC 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
F 
0. 
I 
0 
  VARIABLE   
DESCRIPTION
SLSFAC 
Scale factor for sliding interface penalties, SLSFAC: 
EQ.0: default = .1. 
RWPNAL 
Scale  factor  for  rigid  wall  penalties,  which  treat  nodal  points
interacting  with  rigid  walls,  RWPNAL.    The  penalties  are  set  so
that  an  absolute  value  of  unity  should  be  optimal;  however,  this 
penalty  value  may  be  very  problem  dependent. 
  If  rig-
id/deformable materials switching is used, this option should be
used if the switched materials are interacting with rigid walls. 
LT.0.0:  all  nodes  are  treated  by  the  penalty  method.    This  is 
required for implicit calculations.  Since seven (7) vari-
ables  are  stored  for  each  slave  node,  only  the  nodes
that  may  interact  with  the  wall  should  be  included  in
the node list. 
EQ.0.0: the  constraint  method  is  used  and  nodal  points  which
belong to rigid bodies are not considered. 
GT.0.0:  rigid  bodies  nodes  are  treated  by  the  penalty  method
and all other nodes are treated by the constraint meth-
od. 
ISLCHK 
Initial  penetration  check  in  contact  surfaces  with  indication  of
initial penetration in output files : 
EQ.0: the default is set to 1, 
EQ.1: no checking, 
EQ.2: full check of initial penetration is performed.
VARIABLE   
SHLTHK 
DESCRIPTION
Flag  for  consideration  of  shell  thickness  offsets  in  non-automatic 
surface-to-surface  and  non-automatic  nodes-to-surface 
type 
contacts.    Shell  thickness  offsets  are  always  included  in  single
surface,  constraint-based,  automatic  surface-to-surface,  and 
automatic nodes-to-surface contact types : 
EQ.0: thickness is not considered, 
EQ.1: thickness is considered but rigid bodies are excluded, 
EQ.2: thickness is considered including rigid bodies. 
PENOPT 
Penalty  stiffness  value  option.    For  default  calculation  of  the
penalty value please refer to the LS-DYNA Theory Manual. 
EQ.0: the default is set to 1, 
EQ.1: minimum of master segment and slave node (default for
most contact types), 
EQ.2: use master segment stiffness (old way), 
EQ.3: use slave node value, 
EQ.4: use slave node value, area or mass weighted, 
EQ.5: same  as  4  but  inversely  proportional  to  the  shell
thickness.    This  may  require  special  scaling  and  is  not
generally recommended. 
Options 4 and 5 can be used for metal forming calculations. 
THKCHG 
Shell thickness changes considered in single surface contact: 
EQ.0: no consideration (default), 
EQ.1: shell thickness changes are included. 
ORIEN 
Optional  automatic  reorientation  of  contact  interface  segments
during initialization.  See Remark 4. 
EQ.0: default is set to 1. 
EQ.1: active for automated (part) input only.  Contact surfaces
are given by *PART definitions. 
EQ.2: active for manual (segment) and automated (part) input.
EQ.3: inactive for non-forming contact. 
EQ.4: inactive  for  *CONTACT_FORMING  types  and  *CON-
TACT_DRAWBEAD.
ENMASS 
USRSTR 
USRFRC 
NSBCS 
*CONTROL_CONTACT 
DESCRIPTION
Treatment  of  the  mass  of  eroded  nodes  in  contact.    This  option
affects  all  contact  types  where  nodes  are  removed  after
surrounding  elements  fail.    Generally,  the  removal  of  eroded
nodes  makes  the  calculation  more  stable;  however,  in  problems
where  erosion  is  important  the  reduction  of  mass  will  lead  to
incorrect  results.    ENMASS  is  not  supported  when  SOFT = 2  on 
optional card A. 
EQ.0: eroding nodes are removed from the calculation. 
EQ.1: eroding  nodes  of  solid  elements  are  retained  and
continue to be active in contact. 
EQ.2: the  eroding  nodes  of  solid  and  shell  elements  are
retained and continue to be active in contact. 
Storage  per  contact  interface  for  user  supplied  interface  control
subroutine, see Appendix F.  If zero, no input data is read and no
interface storage is permitted in the user subroutine.  This storage
should  be  large  enough  to  accommodate  input  parameters  and
any history data.  This input data is available in the user supplied
subroutine. 
Storage  per  contact  interface  for  user  supplied  interface  friction
subroutine, see Appendix G.  If zero, no input data is read and no 
interface storage is permitted in the user subroutine.  This storage
should  be  large  enough  to  accommodate  input  parameters  and
any history data.  This input data is available in the user supplied
subroutine. 
Number  of  cycles  between  contact  searching  using  three
dimensional bucket searches, defaults recommended.  For Mortar
contact (option MORTAR on the CONTACT card), the default is
100. 
INTERM 
Flag  for  intermittent  searching  in  old  surface-to-surface  contact 
using the interval specified as NSBCS above: 
EQ.0: off, 
EQ.1: on.
VARIABLE   
XPENE 
DESCRIPTION
Contact  surface  maximum  penetration  check  multiplier.    If  the
small  penetration  checking  option,  PENCHK,  on  the  contact
surface control card is active, then nodes whose penetration then
exceeds the product of XPENE and the element thickness are set
free, see *CONTACT_OPTION_… 
EQ.0: default is set to 4.0. 
SSTHK 
Flag  for  using  actual  shell  thickness  in  single  surface  contact
logic-types 4, 13, 15 and 26.  See Remarks 1 and 2. 
EQ.0: Actual  shell  thickness  is  not  used  in  the  contacts.
(default), 
EQ.1: Actual shell thickness is used in the contacts.  (sometimes
recommended for metal forming calculations). 
ECDT 
Time step size override for eroding contact: 
EQ.0: contact time size may control Dt. 
EQ.1: contact is not considered in Dt determination. 
TIEDPRJ 
Bypass projection of slave nodes to master surface in types: 
*CONTACT_TIED_NODES_TO_SURFACE 
*CONTACT_TIED_SHELL_EDGE_TO_SURFACE 
*CONTACT_TIED_SURFACE_TO_SURFACE 
Tied interface options: 
EQ.0: eliminate gaps by projection nodes, 
EQ.1: bypass projection: Gaps  create 
rotational  constraints 
which can substantially affect results. 
SFRIC 
Default static coefficient of friction  
DFRIC 
Default dynamic coefficient of friction  
EDC 
VFC 
TH 
Default exponential decay coefficient  
Default viscous friction coefficient  
Default contact thickness  
TH_SF 
Default thickness scale factor
VARIABLE   
DESCRIPTION
PEN_SF 
Default local penalty scale factor  
PTSCL 
IGNORE 
Scale factor on the contact stress exerted onto shells formulations
25, 26, and 27.  When DOF = 3 the scale factor also applies to shell 
formulations 2, and 16. 
Ignore  initial  penetrations  in  the  *CONTACT_AUTOMATIC 
options.  In the SMP contact this flag is not implement for the AU-
TOMATIC_GENERAL  option.    “Initial”  in  this  context  refers  to 
the  first  timestep  that  a  penetration  is  encountered.    This  option
can also be specified for each interface on the third optional card
under the keyword, *CONTACT.  The value defined here will be 
the default. 
EQ.0: move nodes to eliminate initial penetrations in the model
definition. 
EQ.1: allow  initial  penetrations  to  exist  by  tracking  the  initial
penetrations. 
EQ.2: allow  initial  penetrations  to  exist  by  tracking  the  initial 
penetrations.    However,  penetration  warning  messages
are printed with the original coordinates and the recom-
mended coordinates of each slave node given. 
FRCENG 
Flag to activate the calculation of frictional sliding energy: 
EQ.0: do not calculate, 
EQ.1: calculate  frictional  energy  in  contact  and  store  as
“Surface  Energy  Density”  in  the  binary  INTFOR  file.
Convert mechanical frictional energy to heat when doing
a  coupled  thermal-mechanical  problem.    When  PKP_-
SEN = 1 on the keyword card *DATABASE_EXTENT_BI-
NARY, it is possible to identify the energies generated on
the upper and lower shell surfaces, which is important in
metal  forming  applications.    This  data  is  mapped  after
each H-adaptive remeshing. 
EQ.2: Same as behavior as above (set to 1) except that frictional
energy is not converted to heat.
VARIABLE   
DESCRIPTION
SKIPRWG 
Flag not to display stationary rigid wall by default. 
EQ.0: generate  4  extra  nodes  and  1  shell  element  to  visualize
stationary planar rigid wall. 
EQ.1: do not generate stationary rigid wall. 
OUTSEG 
Flag  to  output  each  beam  spot  weld  slave  node  and  its  master
segment  for  contact  type:  *CONTACT_SPOTWELD  into  the 
d3hsp file. 
EQ.0: no, do not write out this information. 
EQ.1: yes, write out this information. 
SPOTSTP 
If  a  spot  weld  node  or  face,  which  is  related  to  a  *MAT_-
SPOTWELD beam or solid element, respectively, cannot be found
on the master surface, should an error termination occur? 
SPOTDEL 
EQ.0: no, silently delete the weld and continue, 
EQ.1: yes, print error message and terminate, 
EQ.2: no, delete the weld, print a message, and continue, 
EQ.3: no,  keep  the  weld.    This  is  not  recommended  as  it  can
lead to instabilities. 
This  option  controls  the  behavior  of  spotwelds  when  the  parent
element  erodes.    When  SPOTDEL  is  set  to  1,  the  beam  or  solid
spotweld is deleted and the tied constraint is removed when the
parent  element  erodes.    Parent  element  is  the  element  to  which
the  slave  node  is  attached  using  the  TIED  interface.    This  option
also works for SPRs, i.e.  they automatically fail if at least one of
the  parent  elements  fails.    To  avoid  instabilities,  this  option  is
recommended to be set to 1 for any situation in which the parent 
element is expected to erode. 
EQ.0:  no, do not delete the spot weld beam or solid element or
SPR, 
EQ.1:  yes, delete the weld elements or SPRs when the attached
shells on one side of the element fail. 
On vector processors this option can significantly slow down the 
calculation if many weld elements fail since the vector lengths are
reduced.  On non-vector processors the cost-penalty is minimal.
SPOTHIN 
*CONTROL_CONTACT 
DESCRIPTION
Optional  thickness  scale  factor.    If  active,  define  a  factor  greater
than zero, but less than one.  Premature failure of spot welds can 
occur due to contact of the spot welded parts in the vicinity of the
spot weld.  This contact creates tensile forces in the spot weld. 
Although  this  may  seems  physical,  the  compressive  forces
generated  in  the  contact  are  large  enough  to  fail  the  weld  in 
tension before failure is observed in experimental test.  With this
option,  the  thickness  of  the  parts  in  the  vicinity  of  the  weld  are
automatically  scaled,  the  contact  forces  do  not  develop,  and  the
problem is avoided.  We recommend setting the IGNORE option 
to  1  or  2  if  SPOTHIN  is  active.    This  option  applies  only  to  the
AUTOMATIC_SINGLE_SURFACE option.  See Remark 5. 
ISYM 
Symmetry plane option default for automatic segment generation 
when contact is defined by part ID’s: 
EQ.0: off, 
EQ.1: do  not  include  faces  with  normal  boundary  constraints
(e.g., segments of brick elements on a symmetry plane). 
This option is important to retain the correct boundary conditions
in the model with symmetry. 
NSEROD 
Flag to use one-way node to surface erosion 
EQ.0: use two-way algorithm 
EQ.1: use one-way algorithm 
RWGAPS 
Flag  to  add  rigid  wall  gap  stiffness,  see  parameter  RWGDTH
below. 
EQ.1: add gap stiffness 
EQ.2: do not add gap stiffness 
RWGDTH 
RWKSF 
Death time for gap stiffness.  After this time the gap stiffness is no
longer added. 
Rigid  wall  penalty  scale  factor  for  contact  with  deformable  parts
during  implicit  calculations.    This  value  is  independent  of  SLS-
FAC  and  RWPNAL.    If  RWKSF  is  also  specified  in  *RIGID-
WALL_PLANAR, the stiffness is scaled by the product of the two
values.
VARIABLE   
ICOV 
DESCRIPTION
the 
covariant 
Invokes 
formulation  of  Konyukhov  and
Schweizerhof  in  the  FORMING  contact  option.    This  option  is
available  in  the  third  revision  of  version  971,  but  is  not 
recommended since it is still being implemented. 
EQ.0: standard formulation (default) 
EQ.1: covariant contact formulation. 
SWRADF 
Spot weld radius scale factor for neighbor segment thinning 
EQ.0: neighbor segments not thinned (default) 
GT.0:  The  radius  of  beam  spot  welds  are  scaled  by  SWRADF
when searching for close neighbor segments to thin. 
ITHOFF 
Flag  for  offsetting  thermal  contact  surfaces  for  thick  thermal
shells 
EQ.0: No  offset,  if  thickness  is  not  included  in  the  contact  the 
heat will be transferred between the mid-surfaces of the 
corresponding contact segments (shells). 
EQ.1: Offsets are applied so that contact heat transfer is always
between  the  outer  surfaces  of  the  contact  segments
(shells). 
SHLEDG 
Flag  for  assuming  edge  shape  for  shells  when  measuring
penetration.    This  is  available  for  segment  based  contact   
EQ.0: Shell edges are assumed round (default), 
EQ.1: Shell  edges  are  assumed  square  and  are  flush  with  the
nodes 
PSTIFF 
Flag  to  choose  the  method  for  calculating  the  penalty  stiffness.
This  is  available  for  segment  based  contact  .  See Remark 6. 
EQ.0: Based  on  material  density  and  segment  dimensions
(default), 
EQ.1: Based on nodal masses.
VARIABLE   
DESCRIPTION
ITHCNT 
Thermal contact heat transfer methodology 
LT.0:  conduction evevenly distributed (pre R4) 
EQ.0: default set to 1 
EQ.1: conduction  weighted  by  shape 
functions,  reduced
intergration 
EQ.2: conduction weighted by shape functions, full integration
TDCNOF 
Tied constraint offset contact update option. 
EQ.0: Update velocities and displacements from accelerations 
EQ.1: Update  velocities  and  accelerations  from  displacements.
This  option  is  recommended  only  when  there  are  large
angle  changes  where  the  default  does  not  maintain  a
constant offset to a small tolerance.  This latter option is
not  as  stable  as  the  default  and  may  require  additional
damping for stability.  See *CONTROL_BULK_VISCOSI-
TY and *DAMPING_PART_STIFFNESS. 
Option to output contact forces to RCFORC for all 2 surface force
transducers  when  the  force  transducer  surfaces  overlap.    See
Remark 7. 
EQ.0: Output  to  the  first  force  transducer  that  matches
(default) 
EQ.1: Output to all force transducers that match. 
FTALL 
SHLTRW 
Optional  shell  thickness  scale  factor  for  contact  with  rigid  walls.
Shell  thickness  is  not  considered  when  SHLTRW = 0  (default). 
SHLTRW = 0.5 will result in an offset of half of shell thickness in
contact with rigid walls. 
IGACTC 
Options  to  use  isogeometric  shells  for  contact  detection  when
contact involves isogeometric shells: 
EQ.0: contact  between  interpolated  nodes  and  interpolated
shells 
EQ.1: contact  between  interpolated  nodes  and  isogeometric
shells
*CONTROL 
1.  Shell  Thickness.    The  shell  thickness  change  option  (ISTUPD)  must  be 
activated  in  *CONTROL_SHELL  and  a  nonzero  flag  specified  for  SHLTHK 
above  before  the  shell  thickness  changes  can  be  included  in  the  surface-to-
surface contact types.  If thickness changes are to be included in the single sur-
face  contact  algorithms,  an  additional  flag  must  be  set,  see  THKCHG  above.  
Although  the  contact  algorithms  that  include  the  shell  thickness  are  relatively 
recent, they work in parallel (MPI) Dyna are fully optimized.  The searching in 
these  algorithms  is  considerably  more  extensive  and  therefore  slightly  more 
expensive. 
2.  Upper Limit on Thickness.  In the single surface contacts types SINGLE_SUR-
FACE,  AUTOMATIC_SINGLE_SURFACE,  AUTOMATIC_GENERAL,  AU-
TOMATIC_GENERAL_INTERIOR  and  ERODING_SINGLE_SURFACE,  the 
default contact thickness is taken as the smaller of two values — the shell thick-
ness  or  40%  of  the  minimum  edge  length.    (NOTE:  Minimum  edge  length  is 
calculated  as  min(N4-to-N1,  N1-to-N2,  N2-to-N3).    N3-to-N4  is  neglected  ow-
ing to the possibility of the shell being triangular.) This may lead to unexpected 
results  if  it  is  the  intent  to  include  thickness  effects  when  the  in-plane  shell 
element dimensions are less than the thickness.  The default is based on years of 
experience where it has been observed that sometimes rather large nonphysical 
thicknesses  are  specified  to  achieve  high  stiffness  values.    Since  the  global 
searching algorithm includes the effects of shell thicknesses, nonphysical thick-
ness dimensions slow the search down considerably. 
3. 
Initial  Penetration  Check.    As  of  version  950  the  initial  penetration  check 
option  is  always  performed  regardless  of  the  value  of ISLCHK.    If you  do  not 
want  to  remove  initial  penetrations  then  set  the  contact  birth  time  so that the contact is not active at time 0. 
4.  Automatic  Reorientation.    Automatic  reorientation  requires  offsets  between 
the master and slave surface segments.  The reorientation is based on segment 
connectivity and, once all segments are oriented consistently based on connec-
tivity,  a  check  is  made  to  see  if  the  master  and  slave  surfaces  face  each  other 
based on the right hand rule.   If not, all segments in a given surface are reori-
ented.  This procedure works well for non-disjoint surfaces.  If the surfaces are 
disjoint,  the  AUTOMATIC  contact  options,  which  do  not  require  orientation, 
are  recommended.    In  the  FORMING  contact  options  automatic  reorientation 
works for disjoint surfaces. 
5.  Neighbor  Segment  Thinning  Option.    If  SPOTHIN  is  greater  than  zero  and 
SWRADF  is  greater  than  zero,  a  neighbor  segment  thinning  option  is  active.  
The  radius  of  a  beam  spot  weld  is  scaled  by  SWRADF,  and  then  a  search  is
made  for  shell  segments  that  are  neighbors  of  the  tied  shell  segments  that  are 
touched by the weld but not tied by it. 
6.  Segment Masses for Penalty Stiffness.  Segment based contact   calculates  a  penalty  stiffness  based  on  the  solution  time  step 
and  the  masses  of  the  segments  in  contact.    By  default,  segment  masses  are 
calculated  using  the  material  density  of  the  element  associated  with  the  seg-
ment and the volume of the segment.  This method does not take into account 
added  mass  introduced  by  lumped  masses  or  mass  scaling  and  can  lead  to 
stiffness  that  is  too  low.    Therefore,  a  second  method  (PSTIFF = 1)  was  added 
which  estimates  the  segment  mass  using  the  nodal  masses.    Setting  a  PSTIFF 
values here will set the default values for all interfaces.  The PSTIFF option can 
also be specified for individual contact interfaces by defining PSTIFF on option-
al card F of *CONTACT. 
7.  Force Transducer Search Option.  Two surface force transducers measure the 
contact force from any contact interfaces that generate force between the slave 
and master surfaces of the force transducer.  When contact is detected, a search 
is made to see if the contact force should be added to any 2 surface force trans-
ducers.  By default, when a force transducer match is found, the force is added 
and the search terminates.  When FTALL = 1, the search continues to check for 
other  two  surface  force  transducer  matches.    This  option  is  useful  when  the 
slave and master force transducer surfaces overlap.  If there is no  overlap, the 
default is recommended.
*CONTROL 
Purpose:  Change defaults for MADYMO3D/CAL3D coupling, see Appendix I. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
UNLENG 
UNTIME 
UNFORC 
TIMIDL 
FLIPX 
FLIPY 
FLIPZ 
SUBCYL 
Type 
F 
Default 
1. 
F 
1. 
F 
1. 
F 
0. 
I 
0 
I 
0 
I 
0 
I 
1 
  VARIABLE   
UNLENG 
UNTIME 
UNFORC 
TIMIDL 
FLIPX 
DESCRIPTION
Unit  conversion  factor  for  length.    MADYMO3D/GM-CAL3D 
lengths are multiplied by UNLENG to obtain LS-DYNA lengths. 
Unit  conversion  factor  for  time,  UNTIME.    MADYMO3D/GM-
CAL3D time is multiplied by UTIME to obtain LS-DYNA time. 
Unit  conversion  factor  for  force,  UNFORC.    MADYMO3D/GM-
CAL3D  force  is  multiplied  by  UNFORC  to  obtain  LS-DYNA 
force. 
Idle  time  during  which  CAL3D  or  MADYMO  is  computing  and
LS-DYNA remains inactive.  Important for saving computer time.
Flag  for  flipping  X-coordinate  of  CAL3D/MADYMO3D  relative 
to the LS-DYNA model: 
EQ.0: off, 
EQ.1: on. 
FLIPY 
Flag  for  flipping  Y-coordinate  of  CAL3D/MADYMO3D  relative 
to the LS-DYNA model: 
EQ.0: off, 
EQ.1: on. 
FLIPZ 
Flag  for  flipping  Z-coordinate  of  CAL3D/MADYMO3D  relative 
to the LS-DYNA model: 
EQ.0: off, 
EQ.1: on.
VARIABLE   
DESCRIPTION
SUBCYL 
CAL3D/MADYMO3D subcycling interval (# of cycles): 
EQ.0: Set to 1, 
GT.0:  SUBCYL  must  be  an  integer  equal  to  the  number  of  LS-
DYNA  time  steps  between  each  CAL3D/MADYMO3D 
step.  Then the position of the contacting rigid bodies  is
assumed to be constant for n LS-DYNA time steps.  This 
may result in some increase in the spikes in contact, thus
this  option  should  be  used  carefully. 
the
CAL3D/MADYMO3D  programs  usually  work  with  a 
very small number of degrees of freedom, not much gain
in efficiency can be achieved. 
  As
*CONTROL 
Purpose:  Global control parameters for CPM (Corpuscular Particle Method). 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CPMOUT 
NP2P 
NCPMTS  CPMERR 
SFFDC 
Type 
I 
Default 
11 
I 
5 
I 
0 
I 
0 
F 
1.0 
  VARIABLE   
DESCRIPTION
CPMOUT 
Control CPM output database to the d3plot files:  
EQ.11:  full CPM database in version 3 format (default) 
EQ.21:  full CPM database in version 4 format 
EQ.22:  CPM coordinates only in version 4 format 
EQ.23:  CPM summary only in version 4 format 
NP2P 
Number of cycles for repartition particle among processors.  This 
option is only used in LS-DYNA/MPP.  (Default = 5) 
NCPMTS 
Time step size estimation: 
EQ.0: not consider CPM (default) 
EQ.1: use 1 micro-second as CPM time step size.  This provides 
a better time step size if the model is made by rigid body.
CPMERR 
EQ.0: disable  checking  and  only  output  warning  messages
(Default) 
EQ.1:  enable error checking.  If LS-DYNA detects any problem, 
it will either error terminate the job or try to fix the prob-
lem.  Activated checks include: 
1.  Airbag integrity  
2.  Chamber  integrity:    this  step  applies  the  airbag 
integrity check to the chamber. 
3. 
Inconsistent orientation between the shell refer-
VARIABLE   
DESCRIPTION
SFFDC 
Scale  factor  for  the  force  decay  constant.    The  default  value  is  1
and allowable arrange is [0.01,100].   
ence geometry and FEM shell connectivity. 
Remarks: 
1.  D3PLOT Version.  “Version 3” is an older format than “Version 4”.  Version 4 
stores  data  more  efficiently  than  version  3  and  has  options  for  what  data  is 
stored, but may not be readable by old LS-PrePost executables. 
2.  Airbag Integrity Checking.  The bag’s volume is used to evaluate all bag state 
variables.    If  the  volume  is  ill-defined  or  inaccurate,  then  the  calculation  will 
fail.  Therefore, it is vital that that the volume be closed, and that all shell nor-
mal vectors point in the same direction.   
When  CPMERR = 1  the  calculation  will  error  terminate  if  either  the  bag’s  vol-
ume is not closed or if one of its parts is not internally oriented (meaning that it 
contains  elements  that  are  not  consistently  oriented).    Once  it  is  verified  that 
each  part  has  a  well-defined  orientation,  an  additional  check  is  performed  to 
verify that all of bag’s constituent parts are consistently oriented with respect to 
each other.  If they are not, then the part orientations are flipped until the bag is 
consistently oriented with an inward pointing normal vector. 
3.  Force  Decay  Constant.    Particle  impact  force  is  gradually  applied  to  airbag 
segment by a special smoothing function with the following form. 
𝐹apply = [1 − exp (
−𝑑𝑡
SFFDC× 𝜏
)] (𝐹current + 𝐹stored) 
Where τ is the force decay constant stored in LS-DYNA.
Purpose:  Control CPU time. 
*CONTROL 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CPUTIM 
IGLST 
Type 
F 
I 
  VARIABLE   
DESCRIPTION
CPUTIM 
Seconds of CPU time: 
EQ.0.0: no CPU time limit set  
GT.0.0:  time limit for cumulative CPU of the entire simulation,
including all restarts. 
LT.0.0:  absolute value is the CPU time limit in seconds for the
first run and for each subsequent restart. 
IGLST 
Flag for outputting CPU and elapsed times in the “glstat” file 
EQ.0: no 
EQ.1: yes 
Remarks: 
The CPU limit is not checked until after the initialization stage of the calculation.  Upon 
reaching  the  CPU  limit,  the  code  will  output  a  restart  dump  file  and  terminate.    The 
CPU limit can also be specified on the LS-DYNA execution line via “c=”.  If a value is 
specified on both the execution line and in the input deck, the minimum value will be 
used.
*CONTROL_DEBUG 
Purpose:    Write  supplemental  information  to  the  messag  file(s).    One  effect  of  this 
command  is  that  the  sequence  of  subroutines  called  during  initialization  and  memory 
allocation is printed.  Aside from that, the extra information printed pertains only to a 
select few features, including: 
1.  Spot  weld  connections  which  use  *MAT_100_DA  and  *DEFINE_CONNEC-
TION_PROPERTIES. 
2.  The  GISSMO  damage model  invoked  using  *MAT_ADD_EROSION.    (Supple-
mental information about failed elements is written.)
*CONTROL_DISCRETE_ELEMENT 
Purpose:  Define global control parameters for discrete element spheres. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NDAMP 
TDAMP 
FRICS 
FRICR 
NORMK 
SHEARK 
CAP 
VTK 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
F 
0.01 
2/7 
I 
0 
I 
0 
Capillary Card.  Additional card for CAP ≠ 0.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
GAMMA 
VOL 
ANG 
GAP 
NBUF 
PARALLEL
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
I 
6 
I 
0 
Card 3 is optional.  If optional Card 3 is used, then Optional Card 2 must be defined. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LNORM 
LSHEAR 
FRICD 
DC 
Type 
Default 
I 
0 
I 
0 
F 
FRICS 
F 
0 
  VARIABLE   
DESCRIPTION
NDAMP 
Normal damping coefficient 
TDAMP 
Tangential damping coefficient
r1
r2
X1
X2
Figure 12-12.  Schematic representation of sphere-sphere interaction 
  VARIABLE   
DESCRIPTION
FRICS 
Static coefficient of friction 
EQ.0: 3 DOF 
NE.0:  6 DOF (consider rotational DOF) 
FRICR 
Rolling friction coefficient 
NORMK 
Optional:  scale  factor  of  normal  spring  constant.    Norm  contact
stiffness  is  calculated  as  𝐾𝑛 =
(Default = 0.01)  
{⎧ 𝑘1𝑟1𝑘2𝑟2
𝑘1𝑟1+𝑘2𝑟2
⎩{⎨
|𝑁𝑂𝑅𝑀𝐾|                𝑖𝑓  𝑁𝑂𝑅𝑀𝐾 < 0
𝑁𝑂𝑅𝑀𝐾   𝑖𝑓  𝑁𝑂𝑅𝑀𝐾 > 0
SHEARK 
Optional:  ratio  between  SHEARK/NORMK  (Default = 2/7). 
Tangential stiffness is calculated as 𝐾𝑡 = 𝑆𝐻𝐸𝐴𝑅𝐾 ∙ 𝐾𝑛  
CAP 
EQ.0: dry particles 
NE.0:  wet  particles,  consider  capillary 
additional input card.  See Remark 1. 
force  and  need
VTK 
Output DES in VTK format for ParaView 
EQ.0: no 
EQ.1: yes 
GAMMA 
Liquid surface tension, 𝛾 
VOL 
Volume fraction
VARIABLE   
DESCRIPTION
ANG 
GAP 
Contact angle, 𝜃 
Optional parameter affecting the spatial limit of the liquid bridge.
CAP.EQ.0: GAP  is  ignored,  if  the  CAP  field  is  0  and  the
simulation is modeling dry particles. 
CAP.NE.0: A  liquid  bridge  exists  when  𝛿,  as  illustrated  in 
Figure  12-13,  is  less  or  equal  to  min(GAP, 𝑑rup)
where 𝑑rup is the rupture distance of the bridge au-
tomatically calculated by LS-DYNA .
NBUF 
GE.0: Factor of memory use for asynchronous message buffer 
(Default = 6) 
LT.0:  Disable  asynchronous  scheme  and  use  minimum
memory for data transfer 
PARALLEL 
EQ.0: skip contact force calculation for bonded DES (Default) 
EQ.1: consider contact force calculation for bonded DES 
LNORM 
LSHEAR 
FRICD 
Load curve ID of a curve that defines function for normal stiffness
with respect to norm penetration ratio.  See Remark 2. 
Load curve ID of a curve that defines function for shear stiffness
with respect to norm penetration ratio.  See Remark 3. 
Dynamic coefficient of friction.  By default, FRICD = FRICS.  The 
frictional  coefficient  is  assumed  to  be  dependent  on  the  relative
velocity  𝑣𝑟𝑒𝑙of  the  two  DEM  in  contact  𝜇𝑐 = 𝐹𝑅𝐼𝐶𝐷 + (𝐹𝑅𝐼𝐶𝑆 −
𝐹𝑅𝐼𝐶𝐷)𝑒−𝐷𝐶∙∣𝑣𝑟𝑒𝑙∣. 
DC 
Exponential  decay  coefficient. 
  The  frictional  coefficient  is 
assumed  to  be  dependent  on  the  relative  velocity  𝑣𝑟𝑒𝑙of  the  two 
DEM in contact 𝜇𝑐 = 𝐹𝑅𝐼𝐶𝐷 + (𝐹𝑅𝐼𝐶𝑆 − 𝐹𝑅𝐼𝐶𝐷)𝑒−𝐷𝐶∙∣𝑣𝑟𝑒𝑙∣.
r1
r2
Figure 12-13.  Schematic representation of capillary force model. 
Background: 
This method models all parts as being comprised of rigid spheres.  These sphere interact 
with  both  conventional  solids  and  other  spheres.    Sphere-sphere  interactions  are 
modeled  in  contact  points  using  springs  and  dampers  as  illustrated  in  Figure  12-12.  
[Cundall & Strack 1979] 
Remarks: 
1.  Capillary  Forces  to  Model  Cohesion.    This  extension  is  enabled  using  the 
CAP  field.    Capillary  force  between  wet  particles  is  based  on  the  following 
reference.  “Capillary Forces between Two Spheres with a Fixed Volume Liquid 
Bridges: Theory and Experiment”, Yakov I.  Rabinovich et al.  Langmuir 2005, 
21, 10992-10997.  See Figure 12-13. 
The capillary force is given by 
where, 
and, 
𝐹 = −
2𝜋𝑅𝛾𝑐𝑜𝑠𝜃
1 + 𝛿
2𝑑
, 
𝑑 =
⎜⎛−1 + √1 +
2 ⎝
2𝑉
𝜋𝑅𝛿2
⎟⎞, 
⎠
𝑅 =
2𝑟1𝑟2
𝑟1 + 𝑟2
. 
2.  For  two  interacting  DEMs  with  user  defined  curve  for  norm  stiffness  y = f(x), 
min (𝑟1,𝑟2)  is  relative  penetration,  and  δ  is  penetration;  the  normal 
where  𝑥 =
spring force is calculated as
𝐹𝑛 = 𝑘𝑒𝑓𝑓 ∙ 𝑦 ∙ 𝑚𝑖𝑛2(𝑟1, 𝑟2) 
        where  𝑘𝑒𝑓𝑓   is  the  effective  bulk  modulus  of  two  interacting  DEM  particles 
.    If  curve  is  defined  as  𝑦 = 𝑐 ∙ 𝑥,  the  behavior  is  the  same  as 
𝑘1𝑘2
𝑘1+𝑘2
𝑘𝑒𝑓𝑓 =
NORMK = c. 
3.  For  two  interacting  DEMs  with  user  defined  curve  for  shear  stiffness  y = f(x), 
where  𝑥 =
min (𝑟1,𝑟2)  is  relative  penetration,  and  δ  is  penetration;  the  tangential 
stiffness  is  calculated  as  𝐾𝑠 = 𝑦 ∙ 𝐾𝑛,  where  𝐾𝑛  is  norm  stiffness  defined  by 
NORMK or user defined curve.  If curved is defined as y = c, the behavior is the 
same as SHEARK = c.
*CONTROL_DYNAMIC_RELAXATION 
Purpose:    Initialize  stresses  and  deformation  in  a  model  to  simulate  a  preload.  
Examples  of  preload  include  load  due  to  gravity,  load  due  to  a  constant  angular 
velocity,  and  load  due  to  torquing  of  a  bolt.    After  the  preloaded  state  is  achieved  by 
one of the methods described below, the time resets to zero and the normal phase of the 
solution automatically begins from the preloaded state.  
IDRFLG controls the manner in which the preloaded state is computed.  If IDRFLG is 1 
or -1, a transient “dynamic relaxation” analysis is invoked in which an explicit analysis, 
damped  by  means  of  scaling  nodal  velocities  by  the  factor  DRFCTR  each  time  step,  is 
performed.    When  the  ratio  of  current  distortional  kinetic  energy  to  peak  distortional 
kinetic energy (the convergence factor) falls below the convergence tolerance (DRTOL) 
or  when  the  time  reaches  DRTERM,  the  dynamic  relaxation  analysis  stops  and  the 
current state becomes the initial state of the subsequent normal analysis.   
Distortional kinetic energy is defined as total kinetic energy less the kinetic energy due 
to rigid body motion.  A history of the distortional kinetic energy computed during the 
dynamic relaxation phase is automatically written to a file called “relax”.  This file can 
be  read  as  an  ASCII  file  by  LS-PrePost  and  its  data  plotted.    The  “relax”  file  also 
includes a history of the convergence factor. 
To  create  a  binary  output  database  having  the  same  format  as  a  d3plot  database  but 
which  pertains  to  the  dynamic  relaxation  analysis,  use  *DATABASE_BINARY_D3-
DRLF.    The  output  interval  is  given  by  this  command  as  an  integer  representing  the 
number  of  convergence  checks  between  output  states. 
  The  frequency  of  the 
convergence checks is controlled by the parameter NRCYCK. 
Dynamic  relaxation  will  be  invoked  if  SIDR  is  set  to  1  or  2  in  any  of  the  *DEFINE_-
CURVE  commands,  even  if  IDRFLG = 0  in  *CONTROL_DYNAMIC_RELAXATION.  
Curves so tagged are applicable to the dynamic relaxation analysis phase.  Curves with 
SIDR  set  to  0  or  2  are  applicable  to  the  normal  phase  of  the  solution.    Dynamic 
relaxation will always be skipped if IDRFLAG is set to -999. 
At  the  conclusion  of  the  dynamic  relaxation  phase  and  before  the  start  of  the  normal 
solution  phase,  a  binary  dump  file  (d3dump01)  and  a  “prescribed  geometry”  file 
(drdisp.sif) are written by LS-DYNA.  Either of these files can be used in a subsequent 
analysis  to  quickly  initialize  to  the  preloaded  state  without  having  to  repeat  the 
dynamic relaxation run.   The binary dump file is utilized via a restart analysis .    The  drdisp.sif  file  is  utilized  by 
setting IDRFLG=2 as described below and discussed in Remark 1. 
If IDRFLG is set to 2, the preloaded state is quickly reached by linearly ramping nodal 
displacements, rotations, and temperatures to prescribed values over 100 time steps, or 
over  a  number  of  time  steps  as  indicated  by  the  variable  NC.    See  the  optional  cards 
pertaining to IDRFLG = 2 and also Remarks 1 and 5.
If IDRFLG is set to 5, an implicit analysis is performed to obtain the preloaded state and 
in  this  case,  the  preload  analysis  completes  when  'time'  is  equal  to  DRTERM.    The 
implicit step size is specified with a *CONTROL_IMPLICIT_GENERAL command.  The 
implicit analysis is, by default, static but can be made transient via the *CONTROL_IM-
PLICIT_DYNAMICS command . 
IDRFLG = 6 also performs an implicit analysis as with IDRFLG = 5 but only for the part 
subset specified with DRPSET. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NRCYCK 
DRTOL 
DRFCTR  DRTERM 
TSSFDR 
IRELAL 
EDTTL 
IDRFLG 
Type 
I 
F 
F 
F 
F 
I 
F 
Default 
250 
0.001 
0.995 
infinity  TSSFAC
0 
0.04 
I 
0 
Remarks 
3 
1, 2, 3 
Additional card for IDRFLG = 3 or 6.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DRPSET 
Type 
Default 
Remarks 
I 
0
3 
4 
5 
6 
7 
8 
Additional card for IDRFLG = 2.  
  Card 2 
Variable 
1 
NC 
Type 
I 
Default 
100 
2 
NP 
I 
0 
NP Additional cards for IDRFLG = 2. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PSID 
VECID 
Type 
Default 
I 
0 
I 
0 
  VARIABLE   
NRCYCK 
DESCRIPTION
Number  of  time  steps  between  convergence  checks  for  explicit
dynamic relaxation. 
DRTOL 
Convergence 
(default = 0.001). 
tolerance 
for 
explicit  dynamic 
relaxation
DRFCTR 
Dynamic relaxation factor (default = .995). 
DRTERM 
TSSFDR 
Optional  termination  time  for  dynamic  relaxation.    Termination
occurs  at  this  time  or  when  convergence  is  attained  (de-
fault = infinity). 
Scale  factor  for  computed  time  step  during  explicit  dynamic
relaxation.  If zero, the value is set to TSSFAC defined on *CON-
TROL_TIMESTEP.    After  converging,  the  scale  factor  is  reset  to
TSSFAC.
VARIABLE   
IRELAL 
DESCRIPTION
Automatic  control  for  dynamic  relaxation  option  based  on 
algorithm of Papadrakakis [1981]: 
EQ.0: not active, 
EQ.1: active. 
EDTTL 
Convergence 
relaxation. 
tolerance  on  automatic  control  of  dynamic
IDRFLG 
Dynamic relaxation flag for stress initialization: 
EQ.-999:  dynamic relaxation not activated even if specified on 
a load curve, see *DEFINE_CURVE. 
EQ.-1: 
dynamic  relaxation  is  activated  and  time  history
output  is  produced  during  dynamic  relaxation,  see
Remark 2. 
EQ.0: 
EQ.1: 
EQ.2: 
EQ.3: 
EQ.5: 
EQ.6  
not active, 
dynamic relaxation is activated, 
initialization to a prescribed geometry, see Remark 1,
dynamic  relaxation  is  activated  as  with  IDRFLG = 1, 
but with a part set ID for convergence checking, 
initialize implicitly, see Remark 3. 
initialize  implicity  but  only  for  the  part  set  specified
by DRPSET. 
DRPSET 
Part set ID for convergence checking (for IDRFLG = 3 or 6 only) 
NC 
NP 
Number of time steps for initializing geometry of IDRFLG = 2. 
Number of part sets specified for IDRFLG = 2. 
PSID 
Part set ID for IDRFLG = 2. 
VECID 
Vector ID for defining origin and axis of rotation for IDRFLG = 2. 
See Remark 5. 
Remarks: 
1.  When IDRFLG = 2, an ASCII file specified by "m=" on the LS-DYNA execution 
line  is  read  which  describes  the  initialized  state.    The  ASCII  file  contains  each
node  ID  with  prescribed  values  of  nodal  displacement  (x,  y,  z),  nodal  rotation 
(x, y, z) and nodal temperature in (I8, 7E15.0) format. 
2. 
If  IDRFLG  is  set  to  -1  the  dynamic  relaxation  proceeds  as  normal  but  time 
history  data  is  written  to  the  d3thdt  file  in  addition  to  the  normal  data  being 
written to the d3drlf file.  At the end of dynamic relaxation, the problem time is 
reset to zero.  However, information is written to the d3thdt file with an incre-
ment to the time value.  The time increment used is reported at the end of dy-
namic relaxation.   
3.  When IDRFLG = 5 or 6, LS-DYNA performs an implicit analysis for the preload 
phase  of  the  simulation.    Parameters  for  controlling  the  implicit  preload  solu-
tion are defined using appropriate *CONTROL_IMPLICIT  keywords to specify 
solver  type,  implicit  time  step,  etc.    When  using  this  option,  one  must  specify 
DRTERM  to  indicate  the  termination  "time"  of  the  implicit  preload  analysis.  
When  DRTERM  is  reached,  the  implicit  preload  phase  terminates  and  LS-DY-
NA  begins  the  next  phase  of  the  analysis  according  to  IMFLAG  in  *CON-
TROL_IMPLICIT_GENERAL.    For  example,  if  it  is  desired  to  run  an  implicit 
preload    phase  and  switch  to  the  explicit  solver  for  the  subsequent  transient 
phase, IDRFLG should be set to 5 and  IMFLAG should be set to 0. 
4.  When IDRFLG = 3, a part set ID is used to check for convergence.  For example, 
if only the tires are being inflated on a vehicle, it may be sufficient in some cases 
to  look  at  convergence  based  on  the  part ID’s  in  the  tire  and  possibly  the  sus-
pension  system.    You  can  also  use  IDRFLG = 6  to  perform  the  initialization 
using implicit on the part set. 
5.  When the displacements for IDRFLG = 2 are associated with large rotations, the 
linear interpolation of the displacement field introduces spurious compression 
and tension into the part.  If a part set is specified  with a vector, the displace-
ment is interpolated by using polar coordinates with the tail of the vector speci-
fying  the  origin  of  the  coordinate  system  and  the  direction  specifying  the 
normal to the polar coordinate plane.
*CONTROL 
Purpose:  Define controls for the mesh-free computation. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ISPLINE 
IDILA 
ININT 
Type 
Default 
I 
0 
I 
0 
Remarks 
  Card 2 
1 
2 
I 
12 
1 
3 
4 
5 
6 
7 
8 
Variable 
IMLM 
ETOL 
IDEB 
HSORT 
SSORT 
Type 
Default 
I 
0 
F 
1.0E-4 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
ISPLINE 
Optional choice for the mesh-free kernal functions: 
EQ.0: Cubic spline function (default) 
EQ.1: Quadratic spline function 
EQ.2: Cubic spline function with circular disk 
IDILA 
Optional choice for the normalized dilation parameter: 
EQ.0: Maximum distance based on the background element 
EQ.1: Maximum distance based on surrounding nodes 
ININT 
This  is  the  factor  needed  for  the  estimation  of  maximum
workspace  (MWSPAC)  that  can  be  used  during  the  initialization
phase.
IMLM 
*CONTROL_EFG 
DESCRIPTION
Optional  choice  for  the  matrix  operation,  linear  solving  and 
memory usage: 
EQ.1: Original BCSLIB-EXT solvers 
EQ.2: EFGPACK 
ETOL 
Error tolerance in the IMLM.  When IMLM = 2 is used, ININT in 
card one becomes redundant.  IMLM = 2 is recommended. 
IDEB 
Output internal debug message 
HSORT 
Not used 
SSORT 
Automatic  sorting  of  background  triangular  shell  elements  to
FEM #2 when EFG shell type 41 is used 
EQ.0: no sorting 
EQ.1: full sorting 
Remarks: 
1.  The mesh-free computation requires calls to use BCSLIB-EXT solvers during the 
initialization  phase.    The  maximum  workspace  (MWSPAC)  that  can  be  used 
during the call is calculated as 
MWSPAC = ININT3 × NUMNEFG, 
where NUMNEFG is the total number of mesh-free nodes.  ININT, which is the 
number of nodes that a node influences along each cardinal direction, defaults 
to 12.  When the normalized dilation parameters (DX, DY, DZ) in *SECTION_-
SOLID_EFG are increased ININT must likewise increase. 
2.  When  ISPLINE = 2  is  used,  the  input  of  the  normalized  dilation  parameters 
(DX,  DY,  DZ)  for  the  kernel  function  in  *SECTION_SOILD_EFG  and  SECTI-
OL_SHELL_EFG only requires the DX value. 
3.  EFGPACK  was  added  to  automatically  compute  the  required  maximum 
workspace  in  the  initialization  phase  and  to  improve  efficiency  in  the  matrix 
operations, linear solving, and memory usage.  The original BCSLIB-EXT solver 
requires an explicit workspace (ININT) for the initialization.
*CONTROL 
Purpose:  Provide controls for energy dissipation options. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
HGEN 
RWEN 
SLNTEN 
RYLEN 
Type 
Default 
I 
1 
I 
2 
I 
1 
I 
1 
  VARIABLE   
HGEN 
DESCRIPTION
Hourglass  energy  calculation  option. 
significant additional storage and increases cost by ten percent: 
  This  option  requires
EQ.1: hourglass energy is not computed (default), 
EQ.2: hourglass  energy  is  computed  and  included  in  the
energy  balance.    The  hourglass  energies  are  reported  in 
files  glstat  and  matsum,  see  *DATA-
the  ASCII 
BASE_OPTION. 
RWEN 
Rigidwall energy (a.k.a.  stonewall energy) dissipation option: 
EQ.1: energy dissipation is not computed, 
EQ.2: energy  dissipation  is  computed  and  included  in  the
energy  balance  (default).    The  rigidwall  energy  dissipa-
tion  is  reported  in  the  ASCII  file  glstat,  see  *DATA-
BASE_OPTION. 
SLNTEN 
Sliding  interface  energy  dissipation  option  (This  parameter  is
always set to 2 if contact is active.  The option SLNTEN = 1 is not 
available.): 
EQ.1: energy dissipation is not computed, 
EQ.2: energy  dissipation  is  computed  and  included  in  the
energy balance.  The sliding interface energy is reported 
in  ASCII 
*DATA-
BASE_OPTION. 
files  glstat  and  sleout, 
see
VARIABLE   
DESCRIPTION
RYLEN 
Rayleigh energy dissipation option (damping energy dissipation):
EQ.1: energy dissipation is not computed (default), 
EQ.2: energy  dissipation  is  computed  and  included  in  the 
energy  balance.    The  damping  energy  is  reported  in
*DATA-
ASCII 
BASE_OPTION. 
  and  matsum, 
file  glstat 
see
*CONTROL_EXPLICIT_THERMAL 
The  *CONTROL_EXPLICIT_THERMAL_SOLVER  keyword  activates  an  explicit  finite 
volume  code  solving  heat  transfers  by  conduction.    Enthalpies  and  temperatures  are 
element  centered.    The  elements  supported  by  the  thermal  solver  are  beams,  shells, 
The 
solids, 
*CONTROL_EXPLICIT_THERMAL_PROPERTIES  keyword  defines  the  heat  capacities 
and  conductivities  by  parts.    These  2  keywords  are  mandatory  to  properly  run  the 
solver.    Other  keywords  can  be  used  to  set  the  initial  and  boundary  conditions  and 
control the outputs.  They are all listed below in alphabetical order: 
multi-material 
elements. 
ALE 
3D 
*CONTROL_EXPLICIT_THERMAL_ALE_COUPLING 
*CONTROL_EXPLICIT_THERMAL_BOUNDARY 
*CONTROL_EXPLICIT_THERMAL_CONTACT 
*CONTROL_EXPLICIT_THERMAL_INITIAL 
*CONTROL_EXPLICIT_THERMAL_OUTPUT 
*CONTROL_EXPLICIT_THERMAL_PROPERTIES 
*CONTROL_EXPLICIT_THERMAL_SOLVER
*CONTROL_EXPLICIT_THERMAL_ALE_COUPLING 
Purpose:  Define the shell and solid parts involved in an explicit finite volume thermal 
requires 
coupling  with  multi-material  ALE 
*CONSTRAINED_LAGRANGE_IN_SOLID, CTYPE = 4.  
keyword 
groups. 
  This 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PARTSET  MMGSET 
Type 
I 
I 
Default 
none 
none 
  VARIABLE   
DESCRIPTION
PARTSET 
Part set ID  
MMGSET 
Multi-material 
MATERIAL_GROUP_LIST) 
set 
ID 
(see 
*SET_MULTI-
Remarks:
*CONTROL_EXPLICIT_THERMAL_BOUNDARY 
Purpose:    Set  temperature  boundaries  with  segment  sets  for  an  explicit  finite  volume 
thermal analysis.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SEGSET 
LCID 
Type 
I 
F 
Default 
none 
none 
  VARIABLE   
DESCRIPTION
SEGSET 
Segment set ID  
LCID 
*DEFINE_CURVE ID defining the temperature in function of time
Remarks: 
1.  Boundary elements.  The boundary temperatures are set at segment centers.  If 
shells or beams have all their nodes in the segment set, these elements would be 
considered  as  boundary  elements:  the  temperatures  at  their  centers  will  be 
controlled by the curve LCID.
*CONTROL_EXPLICIT_THERMAL_CONTACT 
Purpose:    Define  the  beam,  shell  and  solid  parts  involved  in  an  explicit  finite  volume 
thermal contact. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PARTSET  NCYCLE 
Type 
I 
Default 
none 
F 
1 
  VARIABLE   
DESCRIPTION
PARTSET 
Part set ID  
NCYCLE 
Number of cycle between checks of new contact 
Remarks:
*CONTROL_EXPLICIT_THERMAL_INITIAL 
Purpose:    Initialize  the  temperature  centered  in  beams,  shells  or  solids  involved  in  an 
explicit finite volume thermal analysis.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SET 
SETYP 
TEMPINI 
Type 
I 
F 
F 
Default 
none 
none 
0.0 
  VARIABLE   
DESCRIPTION
SET 
set ID 
SETYP 
Type of set: 
EQ.1: solid set 
EQ.2: shell set 
EQ.3:   
TEMPINI 
Initial temperature  
Remarks: 
1.  Material with *EOS.   The  volumetric  enthalpy  is  the  sum  of the  pressure  and 
volumetric internal energy (as defined in *EOS).  If the material has an equation 
of  state,  the  enthalpy  should  not  be  initialized  by  the  temperature  but  by  the 
initial volumetric internal energy and pressure set in *EOS.
*CONTROL_EXPLICIT_THERMAL_OUTPUT 
Purpose:    Output  temperatures  and  enthalpies    for  an  explicit  finite 
volume thermal analysis.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DTOUT  DTOUTYP 
SET 
SETYP 
Type 
F 
Default 
none 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
DTOUT 
Time interval between outputs  
DTOUTYP 
Type of DTOUT: 
EQ.0: DTOUT is a constant 
EQ.1: DTOUT is the ID of *DEFINE_CURVE defining a table of 
time vs DTOUT  
SET 
set ID  
SETYP 
Type of set: 
EQ.1: solid set  
EQ.2: shell set  
EQ.3: beam set . 
2.  Output  by  element.  If  a  set  of  elements  SET  is  defined,  the  temperature  and 
enthalpy  histories  are  output  by  element  in  a  .xy  format.    The  file  names  are
and 
temperature_{beam,shell,solid}ID.xy 
The binary file xplcth_output is not output.
enthalpy_{beam,shell,solid}ID.xy.
*CONTROL_EXPLICIT_THERMAL_PROPERTIES 
Purpose:    Define  the  thermal  properties  of  beam,  shell  and  solid  parts  involved  in  an 
explicit finite volume thermal analysis.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PARTSET 
CP 
CPTYP 
VECID1 
VECID2 
LOCAL 
Type 
I 
F 
Default 
none 
none 
  Card 2 
1 
2 
I 
0 
3 
I 
0 
4 
I 
0 
5 
I 
0 
6 
Variable 
Kxx 
Kxy 
Kxz 
KxxTYP 
KxyTYP 
KxzTYP 
Type 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
  Card 3 
1 
2 
3 
I 
0 
4 
I 
0 
5 
I 
0 
6 
Variable 
Kyx 
Kyy 
Kyz 
KyxTYP 
KyyTYP 
KyzTYP 
Type 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
I 
0 
I 
0 
I 
0 
7 
8 
7
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Kzx 
Kzy 
Kzz 
KzxTYP 
KzyTYP 
KzzTYP 
Type 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
PARTSET 
Part set ID  
CP 
Heat capacity 
CPTYP 
Type of CP: 
EQ.0: CP is a constant 
VECID1, 
VECID2 
EQ.1: CP  is  the  ID  of  *DEFINE_CURVE  defining  a  table  of 
temperature vs heat capacity  
*DEFINE_VECTOR  IDs  to  define  a  specific  coordinate  system.
VECID1  and  VECID2  give  the  𝑥-  and  𝑦-direction  respectively. 
The  𝑧-vector  is  a  cross  product  of  VECID1  and  VECID2.    If  this
latter is not orthogonal to VECID1, its direction will be corrected
with a cross-product of 𝑧- and 𝑥-vectors.  The conductivity matrix 
Kij is applied this coordinate system.  
LOCAL 
Flag to activate an element coordinate system: 
EQ.0: The vectors VECIDj are considered in a global coordinate
system. 
EQ.1: The  vectors  VECIDj  are  considered  in  a  local  system 
attached to the element.  For shells and solids, the system
is  the  same  as  DIREC = 1  and  CTYPE = 12  in  *CON-
STRAINED_LAGRANGE_IN_SOLID.    For  shells,  the 
edge  centers  replace  the  face  centers.    For  beams,  the  𝑥-
in
direction 
*ELEMENT_BEAM  and  there  should  be  a  3rd  node  for 
the 𝑦-direction.      
is  aligned  with 
first  2  nodes 
the 
Kij 
Heat conductivity matrix
VARIABLE   
DESCRIPTION
KijTYP 
Type of Kij: 
EQ.0: Kij is a constant 
EQ.1: Kij  is  the  ID  of  *DEFINE_CURVE  defining  a  table  of 
temperature vs heat conductivity  
Remarks:
*CONTROL_EXPLICIT_THERMAL_SOLVER 
Purpose:    Define  the  beam,  shell  and  solid  parts  involved  in  a  finite  volume  thermal 
analysis.  The enthalpies and temperatures are explicitly updated in time.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PARTSET 
DTFAC 
Type 
I 
F 
Default 
none 
1.0 
  VARIABLE   
DESCRIPTION
PARTSET 
Part set ID  
DTFAC 
Time step factor  
Remarks: 
1.  Time  step.    The  time  step  is  a  minimum  of  the  mechanical  and  thermal  time 
steps.  The thermal time step is a minimum of the element thermal time steps, 
which  are  half  the  enthalpies  divided  by  the  right  hand  side  of the  heat  equa-
tion (conductivity * temperature laplacian).  The thermal time step is scaled by 
DTFAC (=1 by default)
*CONTROL_EXPLOSIVE_SHADOW_{OPTION} 
Available option includes: 
<BLANK> 
SET 
Purpose:  Compute detonation times in explosive elements for which there is no direct 
line  of  sight.    If  this  command  is  not  included  in  the  input,  the  lighting  time  for  an 
explosive element is computed using the distance from the center of the element to the 
nearest  detonation  point,  𝐿𝑑;  the  detonation  velocity,  𝐷;  and  the  lighting  time  for  the 
detonator, 𝑡𝑑: 
𝑡𝐿 = 𝑡𝑑 +
𝐿𝑑
The detonation velocity for this option is taken from the element whose lighting time is 
computed  and  does  not  account  for  the  possibilities  that  the  detonation  wave  may 
travel  through  other  explosives  with  different  detonation  velocities  or  that  the  line  of 
sight may pass outside of the explosive material. 
If this command is present, the lighting time of each explosive element is based on the 
shortest path through the explosive material from the associated detonation point(s) to 
the explosive element.  If inert obstacles exist within the explosive material, the lighting 
time will account for the extra time required for the detonation wave to travel around 
the  obstacles.    The  lighting  times  also  automatically  accounts  for  variations  in  the 
detonation velocity if different explosives are used.   
The  SET  option  requires  input  of  a  set  ID  of  two-dimensional  shell  elements  or  three-
dimensional solid elements for which explosive shadowing is active.  If the SET option 
is  not  used,  Card  1  should  be  omitted  and  shadowing  is  active  for  all  explosive 
elements.  
See also *INITIAL_DETONATION and *MAT_HIGH_EXPLOSIVE.
Card 1.  Card for SET keyword option.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SETID 
Type 
I 
Default 
None 
  VARIABLE   
SETID 
DESCRIPTION
Set  ID  of  a  *SET_SHELL  or  *SET_SOLID.      If  the  SET  option  is
active,  the  lighting  times  are  computed  for  a  set  of  shells
(*SET_SHELL in two dimensions) or solids (*SET_SOLID in three
dimensions).
*CONTROL_FORMING 
Purpose:  Set parameters for metal forming related features. 
*CONTROL_FORMING_AUTOCHECK 
*CONTROL_FORMING_AUTO_NET 
*CONTROL_FORMING_AUTOPOSITION 
*CONTROL_FORMING_BESTFIT 
*CONTROL_FORMING_INITIAL_THICKNESS 
*CONTROL_FORMING_MAXID 
*CONTROL_FORMING_ONESTEP 
*CONTROL_FORMING_OUTPUT 
*CONTROL_FORMING_PARAMETER_READ 
*CONTROL_FORMING_POSITION 
*CONTROL_FORMING_PRE_BENDING 
*CONTROL_FORMING_PROJECTION 
*CONTROL_FORMING_REMOVE_ADAPTIVE_CONSTRAINTS 
*CONTROL_FORMING_SCRAP_FALL 
*CONTROL_FORMING_SHELL_TO_TSHELL 
*CONTROL_FORMING_STONING 
*CONTROL_FORMING_TEMPLATE 
*CONTROL_FORMING_TIPPING 
*CONTROL_FORMING_TOLERANC 
*CONTROL_FORMING_TRAVEL 
*CONTROL_FORMING_TRIM_MERGE 
*CONTROL_FORMING_TRIMMING
*CONTROL_FORMING_UNFLANGING 
*CONTROL_FORMING_USER
*CONTROL_FORMING_AUTOCHECK 
Purpose:    This  keyword  detects  and  corrects  flaws  in  the  mesh  for  the  rigid  body  that 
models  the  tooling.    Among  its  diagnostics  are  checks  for  duplicated  elements, 
overlapping  elements,  skinny/long  elements,  degenerated  elements,  disconnected 
elements, and inconsistent element normal vectors. 
This  feature  also  automatically  orients  each tool’s  element  normal vectors  so  that  they 
face  the  blank.    Additionally  an  offset  can  be  specified  to  create  another  tool  (tool 
physical offset) based on the corrected tool meshes.  Note that this keyword is distinct 
from  *CONTROL_CHECK_SHELL,  which  checks  and  corrects  mesh  quality  problem 
after  trimming,  to  prepare  the  trimmed  mesh  for  the  next  stamping  process.    This 
keyword only applies to shell elements. 
The  tool  offset  feature  is  now  available  in  LS-PrePost  4.2  under  Application  → 
MetalForming → Easy Setup. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ICHECK 
IGD 
IOFFSET 
IOUTPUT 
Type 
Default 
I 
0 
I 
none 
I 
0 
I 
none
VARIABLE   
DESCRIPTION
ICHECK 
Tool mesh checking/correcting flag: 
ICHECK.EQ.0:  Do  not  activate  mesh  checking/correcting
feature. 
ICHECK.EQ.1:  Activate comprehensive mesh check and correct
problematic  tool  meshes  . 
This option reduces the likelihood of unreason-
able  forming  results  and/or  error  termination.
This  is  only  for  regular  forming  simulations.
The calculation will continue after the tool mesh
checking/correcting  phase  is  completed.    See
Example 1. 
The  corrected  tool  meshes  can  be  viewed  and 
recovered from the resulting d3plot files.  If the 
termination  time  is  set  to  “0.0”  or  the  keyword
*CONTROL_TERMINATION  is  absent  all  to-
gether, the simulation will terminate as soon as
checking/correcting  is  completed,  and  correct-
ed tool meshes can be extracted from the d3plot
files. 
IGD 
Not used. 
IOFFSET 
Tool mesh offset flag.  This variable works only when IOUTPUT
is defined, and ICHECK is set to “1”:  
IOFFSET.EQ.0: Do not offset rigid tool mesh.  The sheet blank 
does  not  need  to  be  present.    In  this  case  the
output  files  rigid_offset.inc  and  rigid_offset_
before.inc will be identical.  See Example 2. 
IOFFSET.EQ.1: Perform  rigid  tool  mesh  offset  using  the
variable MST  as specified on 
a  *CONTACT_FORMING_…  card.    The  blank 
must  be  defined  and  positioned  completely
above or below the rigid tool to be offset.  Both
part  ID  and  part  SID  (MSTYP)  can  be  used  in 
defining the MSID.  IOUTPUT must also be de-
fined.
VARIABLE   
DESCRIPTION
IOUTPUT 
Output option flag: 
IOUTPUT.EQ.1: Output offset rigid tool meshes into a keyword
file rigid_offset.inc, and terminates the simula-
tion. 
IOUTPUT.EQ.2: Output  offset  rigid  tool  meshes  as  well  as
nodes  used  to  define  draw  beads  into  a  key-
word  file  rigid_offset.inc,  and  terminates  the 
simulation.  See Example 4. 
IOUTPUT.EQ.3: Output  checked/corrected  tool  as  well  as 
offset rigid tool meshes into two separate key-
word  files,  rigid_offset_before.inc,  and  rigid_
offset.inc,  respectively,  and  terminates  the 
simulation.  See Example 3. 
IOUTPUT.EQ.4: Output  checked/corrected  tool  meshes,  offset 
rigid tool meshes as well as the nodes used to
define  draw  beads  into  two  separate keyword
rigid_
files, 
offset.inc,  respectively,  and  terminates  the 
simulation. 
rigid_offset_before.inc, 
and 
Remarks: 
In sheet metal forming, tools are typically modelled as rigid bodies and their meshes are 
prepared from CAD (IGES or STEP) files according to the following procedure: 
1.  The user imports the CAD data into a preprocessor, such as LS-PrePost. 
2.  The  preprocessor  automatically  generates  a  mesh.    LS-PrePost  features  a 
streamlined GUI for this application. 
3.  Export  the  generated  mesh  to  LS-DYNA  input  files.    The  LS-PrePost  eZ-Setup 
user  interface  provides  quick  access  to  generate  the  necessary  input  files  for 
metal forming applications. 
Ideally,  this  process  should  produce  a  good  mesh  requiring  no  manual  intervention.  
Often,  though,  such  meshes  that  have  been  automatically  generated  from  CAD  data 
have flaws severe enough to prevent an accurate or complete calculation.  This feature, 
*CONTROL_FORMING_AUTOCHECK  is  intended  to  make  LS-DYNA  more  robust 
with respect to tooling mesh quality.
This  keyword  requires that  the  tooling  meshes  represent rigid  bodies.    Also,  when  this 
keyword  is  used,  a  part  ID  or  a  part  set  ID,  corresponding  to  MSTYP = 2  or  3  on  the 
*CONTACT_FORMING_…  card,  may  be  used  to  define  the  master  side,  MSID.  
Segment set ID input, MSTYP = 0, is not supported. 
Some cases of incoming bad tooling meshes which can be corrected by this keyword are 
shown in Figure 12-15.  This keyword can be inserted anywhere in the input deck.  To 
include the corrected tooling mesh into the  d3plot the ICHECK field must be defined.  
The  corrected  mesh  is  written  to  rigid_offset_before.inc  file  if  IOFFSET  and  IOUTPUT 
are defined. 
When  IOFFSET = 1  and  IOUTPUT  is  defined,  the  tool  meshes  will  first  be  checked, 
corrected,  and  reoriented  correctly  towards  the  blank.    Then  the  tool  is  offset  by  an 
amount of 0.5|MST| either on the same or opposite side of the blank, depending on the 
signs  of  the  MST  field  on  the  *CONTACT_FORMING_…  card  (Figure  12-14).    A  new 
keyword  file,  “rigid_offset.inc”  file,  will  be  output  as  containing  the  corrected, 
reoriented, and offset tooling mesh. 
The  tool  offset  feature  is  now  available  in  LS-PrePost  4.2  under  Application  → 
MetalForming  →  Easy  Setup.    The  offset  from  Die  button  under  Binder  can  be  used  to 
create offset tools. 
Note  this  keyword  does  not  work  with  the  SMOOTH  option  in  *CONTACT_FORM-
ING_…  prior to Revision 95456, see Revision information. 
Example 1 - Mesh checking/correction in a regular forming simulation: 
The keyword can be inserted anywhere in a regular forming simulation input deck.  A 
partial input example of checking, correcting the tool meshes and reorienting all tools’ 
normals is provided below.  Note that although MST is defined between blank and die 
contact  interface,  die  meshes  will  not  be  offset,  since  IOFFSET  is  not  defined.  
Simulation  will  continue  if  “&endtime”  is  not  zero,  but  will  terminate  as  soon  as  the 
checking and correcting are done if “&endtime” is set to “0.0”, or *CONTROL_TERMI-
NATION  is  absent  all  together.    Corrected  and  reoriented  tool  meshes  can  be  viewed 
and recovered from d3plot files. 
*KEYWORD 
*INCLUDE 
Tool_blank.k 
*CONTROL_FORMING_AUTOCHECK 
$   ICHECK       IGD   IOFFSET   IOUTOUT 
         1 
*CONTROL_TERMINATION 
&endtime 
⋮  
*CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 
         1  blank to punch 
         1         2         2         2                             1         1 
 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+02          0.0000E+00 0.100E+21
0.000     0.000                 0.0 
*CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 
         2  blank to die                                                         
$     SSID      MSID     SSTYP     MSTYP    SBOXID    MBOXID       SPR       MPR 
         1         3         2         2                             1         1 
$       FS        FD        DC        VC       VDC    PENCHK        BT        DT 
 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+02           0.000E+00 0.100E+21 
$      SFS       SFM       SST       MST      SFST      SFMT       FSF       VSF 
     0.000     0.000              -1.600 
$     SOFT    SOFSCL    LCIDAB    MAXPAR    PENTOL     DEPTH     BSORT    FRCFRQ 
         0 
*CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 
         3  blank to binder 
         1         4         2         2                             1         1 
 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+02           0.000E+00 0.100E+21 
     0.000     0.000                 0.0 
⋮  
*END 
Example  2  -  Mesh  checking/correction  only  for  rigid  tool  mesh  (sheet  blank  not 
required): 
A much shorter but complete input example of checking, correcting the tool meshes and 
reorienting all tools’ normals is shown below.  Note the sheet blank does not need to be 
present,  and  both  rigid_offset.inc  and  rigid_offset_before.inc  will  be  the  same, 
representing  the  checked,  corrected,  and  reoriented  tool  mesh  file,  since  IOFFSET  is 
undefined (no tool offset will be done). 
*KEYWORD 
*INCLUDE 
toolmesh.k 
*CONTROL_FORMING_AUTOCHECK 
$   ICHECK       IGD   IOFFSET   IOUTOUT 
         1                             1 
*PARAMETER_EXPRESSION 
I toolpid          3 
*PART 
$      PID     SECID       MID     EOSID      HGID      GRAV    ADPOPT      TMID 
  &toolpid         2         2                                         
*MAT_RIGID 
$      MID        RO         E        PR         N    COUPLE         M     ALIAS 
         2  7.83E-09  2.07E+05      0.28 
$      CMO      CON1      CON2 
         1         4         7 
$LCO or A1        A2        A3        V1        V2        V3 
*SECTION_SHELL 
$    SECID    ELFORM      SHRF       NIP     PROPT   QR/IRID     ICOMP     SETYP 
         2         2       1.0       3.0       0.0 
$       T1        T2        T3        T4      NLOC 
       1.0       1.0       1.0       1.0 
*END 
Example 3 - Mesh checking/correction and tool offset (sheet blank required): 
In  addition  to  checking,  correcting  and  reorienting  all  tools’  normal,  the  following 
partial input will offset the die meshes in toolmesh.k by 0.88 mm (using the MST value
defined for the die) on the opposite side of the blank, and output the offset tool meshes 
in  a  file rigid_offset.inc.    The  checked/corrected  original  die  meshes  will  be  written to 
rigid_offset_before.inc.    The  simulation  will  terminate  as  soon  as  the  files  are  written, 
regardless of what the “&endtime” value is.  In fact, the keyword *CONTROL_TERMI-
NATION can be omitted all together. 
*KEYWORD 
*INCLUDE 
Tool_blank.k 
*PARAMETER_EXPRESSION 
R blankt         0.8 
R offset        -1.1 
R mst           blankt*offset*2.0 
*CONTROL_FORMING_AUTOCHECK 
$   ICHECK       IGD   IOFFSET   IOUTOUT 
         1                   1         3 
*CONTROL_TERMINATION 
&endtime 
*CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 
         1  blank to punch 
         1         2         2         2                             1         1 
 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+02          0.0000E+00 0.100E+21 
     0.000     0.000                 0.0 
*CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 
         2  blank to die 
$     SSID      MSID     SSTYP     MSTYP    SBOXID    MBOXID       SPR       MPR 
         1         3         2         2                             1         1 
$       FS        FD        DC        VC       VDC    PENCHK        BT        DT 
 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+02           0.000E+00 0.100E+21 
$      SFS       SFM       SST       MST      SFST      SFMT       FSF       VSF 
     0.000     0.000                &mst 
$     SOFT    SOFSCL    LCIDAB    MAXPAR    PENTOL     DEPTH     BSORT    FRCFRQ 
         0 
*CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 
         3  blank to binder 
         1         4         2         2                             1         1 
 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+02           0.000E+00 0.100E+21 
     0.000     0.000                 0.0 
*END 
Example 4 -  Mesh checking/correction and tool offset, bead nodes output (sheet 
blank required): 
In  addition  to  checking,  correcting  and  reorienting  all  tools’  normal,  the  following 
partial input will create an offset tool in the file rigid_offset.inc on the same side of the 
blank; the file will also contain the nodes used to define the contact draw beads #1 and 
#2.  
*KEYWORD 
*INCLUDE 
Tool_blank.k 
R blankt         0.8 
R offset         1.1 
R mst           blankt*offset*2.0 
*CONTROL_FORMING_AUTOCHECK 
$   ICHECK       IGD   IOFFSET   IOUTOUT 
         1                   1         2 
*CONTROL_TERMINATION 
&endtime
*CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 
         1  blank to punch 
         1         2         2         2                             1         1 
 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+02          0.0000E+00 0.100E+21 
     0.000     0.000                 0.0 
*CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 
         2  blank to die 
$     SSID      MSID     SSTYP     MSTYP    SBOXID    MBOXID       SPR       MPR 
         1         3         2         2                             1         1 
$       FS        FD        DC        VC       VDC    PENCHK        BT        DT 
 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+02           0.000E+00 0.100E+21 
$      SFS       SFM       SST       MST      SFST      SFMT       FSF       VSF 
     0.000     0.000                &mst 
$     SOFT    SOFSCL    LCIDAB    MAXPAR    PENTOL     DEPTH     BSORT    FRCFRQ 
         0 
*CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 
         3  blank to binder 
         1         4         2         2                             1         1 
 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+02           0.000E+00 0.100E+21 
     0.000     0.000                 0.0 
⋮  
*CONTACT_DRAWBEAD_ID 
     10001  Draw bead #1 
         1         1         4         2                   0         0         0 
 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+00              0.0615 0.100E+21 
     0.200     0.200 
$   LCIDRF    LCIDNF     DBDTH     DFSCL    NUMINT 
        10         9 0.100E+02 0.700E+00 
*CONSTRAINED_EXTRA_NODES_SET 
        40         1 
*SET_NODE_LIST 
         1 
    915110    915111    915112    915113    915114    915115    915116    915117 
    915118    915119    915120    915121    915122 
*CONTACT_DRAWBEAD_ID 
     10002  Draw bead #2 
         2         1         4         2                   0         0         0 
 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+00              0.0615 0.100E+21 
     0.200     0.200 
$   LCIDRF    LCIDNF     DBDTH     DFSCL    NUMINT 
        11         9 0.100E+02 0.400E+00 
*CONSTRAINED_EXTRA_NODES_SET 
$      PID      NSID 
        40         2 
*SET_NODE_LIST 
         2 
    915123    915124    915125    915126    915127    915128    915129    915130 
    915131    915132    915133    915134    915135    915136    915137 
⋮  
*END 
Revision information: 
This feature is available starting from LS-DYNA Revision 91737, in both SMP, MPP and 
double precision. 
1. 
2. 
IOFFSET, and IOUTPUT = 1 are available starting in Revision 94521.  The latest 
beta revisions should offer better and improved offset meshes. 
IOUTPUT = 2 is available starting in Revision 95357.
3.  Support  of  SMOOTH  contact  option  in  *CONTACT_FORMING...:  is  available 
starting in Revision 95456. 
4. 
IOUTPUT = 3, and 4 are available starting in Revision 96592.
Sheet metal blank must be positioned 
completely above or below the original tool
Original tool (corrected original 
tool in rigid_offset_before.inc) 
A negative MST result in a new  
tool with normal offset distance 
|(0.5)MST| from the original tool, 
on the opposite side of the blank
Offset tool (rigid_offset.inc)
Sheet metal blank must be positioned 
completely above or below the original tool
Offset tool (rigid_offset.inc)
A positive MST result in a new  
tool with normal offset distance 
|(0.5)MST| from the original tool, 
on the same side of the blank
Original tool (corrected original 
tool in rigid_offset_before.inc)
Figure  12-14.    Offset  using  the  MST  value  defined  in  *CONTACT_-
FORMING_…
All nodes of two 
duplicate traingle 
shells 21304, 34630 lie 
in one straight line
Shell 34608 overlaps 
with three other 
triangle shells
Overlapping 
shell 34604
Overlapping 
shell 34607
A severe, multiple overlapping case
A case of typical incoming, inconsistent shell normals
Figure  12-15.    A  few  cases  of  the  tooling  mesh  problems  handled  by  this
keyword.
*CONTROL_FORMING_AUTO_NET 
Purpose:  This keyword is used for simulating springback when the stamping panel is 
resting  on  the  nets  of  a  checking  fixture.    With  this  keyword,  rectangular  nets  are 
automatically generated according to specified dimensions and positions. 
Include one pair of Cards 1 and 2 per net.  Add to the deck as many pairs of cards as 
needed.    This  section  is  terminated  by  the  next  keyword (“*”)  card.    In  general,  for  N 
nets add 2N cards. 
4 
IDP 
I 
0 
4 
8 
5 
X 
F 
6 
Y 
F 
7 
Z 
F 
0.0 
0.0 
0.0 
5 
6 
7 
8 
  Card 1 
1 
2 
3 
Variable 
IDNET 
ITYPE 
IDV 
Type 
I 
Default 
none 
  Card 2 
Variable 
1 
SX 
Type 
F 
2 
SY 
F 
I 
0 
3 
OFFSET 
F 
Default 
0.0 
0.0 
0.0 
VARIABLE 
DESCRIPTION
IDNET 
ID of the net; must be unique. 
ITYPE 
Not used at this time. 
IDV 
Vector ID for surface normal of the net.  See *DEFINE_VECTOR. 
If not defined, the normal vector will default to the global z-axis. 
IDP 
Part ID of the panel undergoing springback simulation. 
X 
Y 
The x-coordinate of a reference point for the net to be generated. 
The y-coordinate of a reference point for the net to be generated.
VARIABLE 
DESCRIPTION
Z 
SX 
SY 
The z-coordinate of a reference point for the net to be generated. 
Length of the net along the first tangential direction.  (The x-axis 
when the normal is aligned along the global z-axis). 
Length  of  the  net  along  the  second  tangential  direction.    (The  y-
axis when the normal is aligned along the global z-axis). 
OFFSET 
The net center will be offset a distance of OFFSET in the direction
of its surface normal.  For positive values, the offset is parallel to
the normal; for negative values, antiparallel. 
General remarks: 
1.  The IDNET field of card 1 sets the “net ID,” which is distinct from the part ID of 
the net; the net ID serves distinguishes this net from other nets. 
2.  The part ID assigned to the net is generated by incrementing the largest part ID 
value in the model.  
3.  Other  properties  such  as  section,  material,  and  contact  interfaces  between  the 
panel and nets are likewise automatically generated. 
4.  The  auto  nets  use  contact  type  *CONTACT_FORMING_ONE_WAY_SUR-
FACE_TO_SURFACE. 
An example: 
The  excerpted  input  file    specifies  four  auto  nets  having  IDs  1  through  4.  
The  vector  with  ID =  89  is  normal  to  the  net.    The  nets  are  offset  4 mm  below  their 
reference points; the direction is below because the normal vector (ID = 89) is parallel to 
the  z-axis  and  the  offset  is  negative.    This  example  input  can  be  readily  adapted  to  a 
typical  gravity-loaded  springback  simulation  obviating  the  need  for  SPC  constraints 
. 
*CONTROL_FORMING_AUTO_NET 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
$    IDNET     ITYPE       IDV       IDP         X         Y         Z 
         1                  89         5   2209.82  -33.6332   1782.48 
$       SX        SY    OFFSET 
      15.0      15.0      -4.0 
$    IDNET     ITYPE       IDV       IDP         X         Y         Z 
         2                  89         5   3060.23  -33.6335   1782.48 
$       SX        SY    OFFSET 
      15.0      15.0      -4.0 
$    IDNET     ITYPE       IDV       IDP         X         Y         Z 
         3                  89         5   3061.21   31.4167   1784.87 
$       SX        SY    OFFSET
Nets automatically 
generated
Two specified 
coordinate locations
Trimmed panel
Figure 12-16.  An example problem. 
      15.0      15.0      -4.0 
$    IDNET     ITYPE       IDV       IDP         X         Y         Z 
         4                  89         5   2208.84   31.4114   1784.87 
$       SX        SY    OFFSET 
      15.0      15.0      -4.0 
*DEFINE_VECTOR 
$ VID, Tail X, Y, Z, Head X, Y, Z 
89,0.0,0.0,0.0,0.0,0.0,100.0 
Discussion of Figures: 
Figure 12-16 shows a formed and trimmed panel of a hat-shaped channel with an auto 
net  at  two  corners.    The  nets  are  offset  4mm  away  from  the  panel.    When  gravity 
loading  is  downward  the  nets  must  be  below  the  panel  (Figure  12-17  left)  so  that  the 
panel comes into contact with the nets after springback as expected (Figure 12-17 right).  
As  shown  in  Figure  12-18  the  situation  must  be  reversed  when  gravity  loading  points 
upward. 
Revision information: 
This  feature  is  now  available  starting  in  implicit  static  in  double  precision  LS-DYNA 
Revision 62781.
Initial OFFSET 4mm 
with gravity load down
Before springback
After springback
Figure 12-17.  Springback and contact with nets - gravity down. 
Initial OFFSET 4mm 
with gravity load up
Before springback
After springback
Figure 12-18.  Springback and contact with nets – gravity up.
*CONTROL_FORMING_AUTOPOSITION_PARAMETER_{OPTION} 
Available options include: 
<BLANK> 
SET 
Purpose:  The purpose of this keyword is to calculate the minimum required separation 
distances  among  forming  tools  for  initial  tool  and  blank  positioning  in  metal  forming 
simulation.  It is applicable to shell elements only.  It does not, actually, move the part; 
for that, see *PART_MOVE. 
NOTE: This keyword requires that model begin in its home 
position.    While  processing  this  card,  LS-DYNA 
moves the parts to match the auto-position results so 
that  auto-position  operations  correctly  compose.  
Upon  completion  of  the  auto-positioning  phase,  the 
parts are returned to their home positions. 
Auto-Position  Part  Cards.    Add  one  card  for  each  part  to  be  auto-positioned.    The 
next keyword (“*”) card terminates this is keyword. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
CID 
DIR 
MPID 
POSITION PREMOVE 
THICK 
PORDER 
Type 
I 
Default 
none 
I 
0 
I 
I 
none 
none 
I 
0 
F 
F 
I/A 
0.0 
0.0 
none 
  VARIABLE   
PID 
DESCRIPTION
Part  ID.    This  part  will  be  moved  based  on  the  following
controlling parameters. 
When  the  option  SET  is  activated,  PID  becomes  part  set  ID,
defined  by  *SET_PART_LIST.    This  is  useful  in  defining  tailor-
welded  blanks,  where  two  pieces  of  the  blank  must  be  moved 
simultaneously.  
CID 
Coordinate ID (Default is global coordinate system).
VARIABLE   
DESCRIPTION
DIR 
Direction in which the part will be moved: 
EQ.1: x direction, 
EQ.2: y direction, 
EQ.3: z direction. 
MPID 
Master  part  ID,  whose  position  is  to  be  referenced  by  PID  for
positioning.    When  the  option  SET  is  activated,  MPID  becomes
part set ID, defined by *SET_PART_LIST. 
POSITION 
Definition of relative position between PID and MPID: 
EQ.1:  PID is above MPID; 
EQ.-1: PID is below MPID. 
Definition  of  “above”  is  determined  by  the  defined  coordinate
system.    If  PID  is  above  MPID,  it  means  PID  has  a  larger  z-
coordinate.  This definition is helpful in line die simulation where
local coordinate system may be used.  
Move  PID  through  distance  PREMOVE  prior  to  processing  the 
other  *CONTROL_FORMING_AUTOPOSITION  cards. 
  See 
Remark 5. 
Thickness  of  the  blank.    The  same  value  must  be  used  in  all
defined move operations under this keyword.  
The  name  of  the  parameter  without  the  ampersand  “&”,  as
defined  in  *PARAMETER,  or  the  position  or  order  of  the
parameter defined in the *PARAMETER list. 
PREMOVE 
THICK 
PORDER 
Background: 
In  line-die  (multi-stage)  simulation,  initial  positioning  of  the  tools  and  blank  is  one  of 
the major issues preventing several die processes from being run automatically from a 
single  job  submission.    The  most  basic  method  for  running  a  line  die  simulation  is  to 
chain a series of calculations together using the previous calculation’s partially formed 
blank, written to a dynain file, as a part of the input for the next calculation. 
Since  the  partial  results  are  not  known  until  the  preceding  calculation  completes,  the 
tools need to reposition before the next calculation.  Without this card the repositioning 
step must be done by-hand using a preprocessor.  With the combination of this card and 
the  LS-DYNA  case  driver    the  repositioning  can  be  fully  automated, 
enabling a complete line-die simulation to be completed with a single job submission.
*CONTROL_FORMING_AUTOPOSITION_PARAMETER 
This card requires that all parts start in their home (tool closed) position.  It calculates 
how far the parts need to be moved to prevent initial penetration.  The results are stored 
into the parameter listed in the PORDER field to be used for a part move operation.  
1.  For  each  defined  move  operation  a  *PARAMETER  card  must  initialize  the 
parameter referred to in the PORDER field. 
2.  All tools must start in home position including desired final gaps. 
3.  The required distance between each contact pair is calculated and stored in the 
initialized parameter named in the PORDER field. 
4.  The parts are repositioned through a distance based on the value written to the 
parameter PORDER using the *PART_MOVE card. 
5.  The  *PARAMETER_EXPRESSION  can  be  used  to  evaluate  expressions 
depending on the move distances, such as times and tool move speeds. 
6.  The *CASE feature, is used to chain together the sub-processes in the line-dime 
simulation. 
Remarks: 
1.  Order  Dependence.    Input  associated  with  this  keyword  is  order  sensitive.  
The following order should be observed: 
a)  All model information including all elements and node 
b)  Part definitions  
c)  Part set definitions  
d)  *PARAMETER initialization 
e)  This keyword 
f)  *PARAMETER_EXPRESSION 
g)  *PART_MOVE 
2.  This  keyword  can  also  be  used  to  generate  a  new  keyword  input  (dynain) 
containing  the  fully  positioned  model  (without  actually  running  the  entire 
simulation).  This procedure is identical to a full calculation except that the *PA-
RAMETER_EXPRESSION  keyword,  the  *CONTROL_TERMINATION  key-
word, and tool kinematic definitions are omitted.
3.  When  working  in  local  coordinate  systems  it  is  often  the  case  that  the  sign  of 
the computed parameter may not correspond to its intended use.  In this case, 
the  absolute  value  function,  ABS,  for  the  *PARAMETER_EXPRESSION  key-
word is especially useful. 
4.  Draw  beads  can  be  modeled  with  beam  elements  that  are  positioned  and 
attached to a tool at home position.  Draw beads with beam elements can also 
be moved in the keyword *PART_MOVE, and automatically positioned just like 
any other types of elements. 
5.  Cards with the PREMOVE field set are processed before all other *CONTROL_-
FORMING_AUTOPOSITON  cards,  regardless  of  their  location  in  the  input 
deck.  The PREMOVE field serves to modify the initial state on which the calcu-
lations of the other AUTOPOSITON cards are based. 
For instance, when a binder is moved downward with the PREMOVE feature, it 
will  be  in  its  post-PREMOVE  position  for  all  other  AUTOPOSITION  calcula-
tions.  But, as is the case with the other AUTOPOSITON cards, the model will 
be  returned  to  its  home  position  upon  completion  of  the  AUTOPOSITION 
phase.    Note  that  the master  part,  MPID,  and  the  POSITION  fields  are  ignored 
when  the  PREMOVE  field  is  set,  and  that  the  PREMOVE  value  is  copied  into 
the PORDER parameter. 
6.  This  feature  is  implemented  in  LS-PrePost4.0  eZSetup  (http://ftp.lstc.com/-
anonymous/  outgoing/lsprepost/4.0/metalforming/)  for  metal  forming  in 
both explicit and implicit application.
Part set 2
(lower binder)
Part set 1
(blank)
Part set 3
(upper die)
Binder PREMOVE 
(183.0 mm)
Initial position
(tools home)
Final position
(after auto-position)
Figure 12-19.  An example of using the variable PREMOVE 
Example 1: 
An air draw process like the one shown in Figure 12-19 provides a clear illustration of 
how  this  card,  and,  in  particular,  the  PREMOVE  field  is  used  to  specify  the  lower 
binder’s travel distance. 
1.  The  card  with  the  PREMOVE  field  set,  the  third  AUTOPOSITON  card,  is 
processed first.  It moves lower binder 183 mm upward from its home position, 
and it will form the base configuration for other AUTOPOSITION cards.  It will 
also  store  this  move  into  &bindmv.    Note  that  although  the  POSITION  and 
MPID fields are set, they are ignored. 
2.  The  first  autoposition  card,  which  will  be  the  second  one  processed,  calculates 
the minimum offset distance (&blankmv) necessary for the blank (part set 1) to 
clear part set 9999, which consists of the lower binder (PID = 2), which is in its 
post-PREMOVE location, and of the lower punch (PID = &lpunid). 
3.  The  next  card  determines  the  minimum  offset  (&updiemv)  necessary  to  bring 
the upper die (part set 3) as close to the blank as possible without penetrating.  
This calculation proceeds under the assumption that the blank part set has been moved 
through &blankmv. 
*SET_PART_LIST 
9999 
&lpunpid,2 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*CONTROL_FORMING_AUTOPOSITION_PARAMETER_SET 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
$      PID       CID       DIR      MPID  POSITION   PREMOVE     THICK    PORDER 
$ blank move 
         1                   3      9999         1             &bthick   blankmv 
$ upper die move 
         3                   3         1         1             &bthick   updiemv 
$ lower binder move 
         2                   3         1        -1     183.0   &bthick    bindmv
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*PART_MOVE 
$    SID            XMOV            YMOV            ZMOV     CID   IFSET 
$ blank move 
       1             0.0             0.0        &blankmv               1 
$ upper die move 
       3             0.0             0.0        &updiemv               1 
$ lower binder move 
       2             0.0             0.0         &bindmv               1 
The following examples demonstrates the *PARAMETER_EXPRESSION card, which is 
used  to  derive  new  parameters  from  the  value  calculated  during  auto-positioning.    In 
this example, the auto-positioned distance for binder, which is stored in the parameter, 
&bindmv, is used to define an additional parameter, 
&bindmv1 = &bindmv − 30 mm 
The  *PART_MOVE  step  uses  &bindmv1  rather  than  &bindmv,  to  move  both  the  lower 
binder and the draw beads. 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*CONTROL_FORMING_AUTOPOSION_PARAMETER_SET 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
$      PID       CID       DIR      MPID  POSITION   PREMOVE     THICK  PORDER 
$ blank move 
   &blksid                   3      9999         1             &bthick   blankmv 
$ upper die move 
  &udiesid                   3   &blksid         1             &bthick   updiemv 
$ lower binder move 
  &bindsid                   3   &blksid        -1             &bthick   bindmv 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8  
*PARAMETER_EXPRESSION 
bindmv1   bindmv-30.0 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*PART_MOVE 
$    SID            XMOV            YMOV            ZMOV     CID   IFSET 
$ blank move 
 &blksid             0.0             0.0        &blankmv               1 
$ upper die move 
&udiesid             0.0             0.0        &updiemv               1 
$ lower binder move 
&bindsid             0.0             0.0        &bindmv1               1 
$ draw beads move 
     909             0.0             0.0        &bindmv1               1
Part set 2
(upper die)
Part set 1
(blank)
&updiemv
&updiemv
&blankmv
&blankmv
Part set 3
(lower binder)
Figure 12-20.  An example of binder closing in air draw 
Example 2: 
Figure 12-20 schematically shows the binder closing in the global Z-direction.  A partial 
keyword details follow.  
*INCLUDE 
$blank from previous case 
case5.dynain 
*INCLUDE 
closing_tool.k 
*INCLUDE 
beads_home.k 
*SET_PART_LIST 
$ blank 
1 
1 
*SET_PART_LIST 
$ upper die 
2 
2 
*SET_PART_LIST 
$ lower binder 
3 
3 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*parameter 
$$$$$$$$$$$$$$$$$$$$$$$$$$ Tool move variables 
R blankmv        0.0 
R updiemv        0.0 
R bindmv         0.0 
$$$$$$$$$$$$$$$$$$$$$$$$$$ Tool speed and ramp up definition 
R tclsup       0.001 
R vcls        1000.0 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*CONTROL_FORMING_AUTOPOSION_PARAMETER_SET 
$      PID       CID       DIR      MPID  POSITION   PREMOVE     THICK  PORDER 
$ positioning blank on top of lower binder 
         1                   3         3         1                 0.7   blankmv 
$ positioning upper die on top of blank 
         2                   3         1         1                 0.7   updiemv 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*PARAMETER_EXPRESSION 
$    PRMR1    EXPRESSION 
R clstime     (abs(updiemv)-vcls*tclsup)/vcls+2.0*tclsup 
R endtime     &clstime 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*PART_MOVE 
$    PID            XMOV            YMOV            ZMOV     CID
1             0.0             0.0        &blankmv 
       2             0.0             0.0        &updiemv 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*CONTROL_TERMINATION 
&endtime 
Revision information: 
This  feature  is  available  starting  in  LS-DYNA  Revision  56080  in  both  explicit  and 
implicit,  SMP  and  MPP  versions.    Later  revisions  are  also  available  with  various 
improvements.
*CONTROL_FORMING_BESTFIT 
Available options include: 
<BLANK> 
VECTOR 
Purpose:    This  keyword  rigidly  moves  a  part  to  the  target  so  that  they  maximally 
coincide.    This  feature  can  be  used  in  sheet  metal  forming  to  translate  and  rotate  a 
spring  back  part  (source)  to  a  scanned  part  (target)  to  assess  spring  back  prediction 
accuracy.    This  keyword  applies  to  shell  elements  only.    The  VECTOR  option  allows 
vector  components  of  the  normal  distance  from  the  target  to  the  part  node  to  be 
included 
keyword 
under 
*NODE_TO_TARGET_VECTOR . 
bestfit.out 
output 
the 
the 
file 
in 
This  feature  is  available  now  in  LS-PrePost  4.3  in  Metal  Forming  Application/eZ  Setup 
(http://ftp.lstc.com/anonymous/outgoing/lsprepost/4.3/win64/). 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IFIT 
NSKIP 
GAPONLY
IFAST 
IFSET 
NSETS 
NSETT 
Type 
Default 
I 
0 
I 
-3 
  Card 2 
1 
2 
I 
0 
3 
Variable 
Type 
Default 
I 
1 
4 
I 
0 
5 
FILENAME 
A80 
none 
I 
I 
none 
none 
6 
7 
8 
  VARIABLE   
DESCRIPTION
IFIT 
Best fit program activation flag: 
IFIT.EQ.0:  do not perform best-fit. 
IFIT.EQ.1:  activate the best-fit program.
VARIABLE   
NSKIP 
DESCRIPTION
Optional  skipping  scheme  during  bucket  searching  to  aid  the
computational speed (zero is no skipping): 
NSKIP.GT.0: Number  of  nodes  to  skip  in  bucket  searching.
NSKIP of  “1”  does  not  skip  any  nodes  in  search-
ing  therefore  computing  speed  is  the  slowest  but
accuracy  is  the  highest.    Higher  values  of  NSKIP
speed  up  the  calculation  time  with  slightly  dete-
riorating accuracies.  Based on studies, a value of
“5”  is  recommended  with  IFAST = 1,  which  bal-
ances the speed and accuracy.  See Table 12-21 for 
the effect of NSKIP on the accuracy of the fitting. 
NSKIP.LT.0:  Absolute  value  is  the  distance  to  skip  in  bucket
searching.  This scheme is faster compared to the
previous  method  and  therefore  is  recommended
for  computational  efficiency  and  accuracy.    A 
value of “-5” is suggested.  See Example 3.
IFAST = 0
IFAST = 1 
NSKIP 
 CPU time 
2 
5 
10 
20 
50 
10 min 38 sec 
4 min 49 sec 
2 min 46 sec 
1 min 24 sec 
50 sec 
Max/Min 
(mm) 
1.28/-1.59 
1.21/-1.59 
1.27/-1.59 
1.27/-1.59 
1.22/-1.61 
 CPU time 
4 min 3 sec 
1 min 59 sec 
1 min 18 sec 
59 sec 
40 sec 
Max/Min 
(mm) 
1.22/-1.59 
1.25/-1.61 
1.44/-1.53 
1.42/-1.64 
1.43/-1.67 
Table  12-21.    Computing  speed  and  the  max/min  deviations  from  the
springback  mesh  to  the  target  scan  for  an  automotive  part,  under  various
combinations  of  NSKIP  and  IFAST.    All  runs  were  made  on  a  1  CPU  XEON
E5520 machine, with 685132 elements on the target  scan and 135635 elements
on the springback mesh. 
  VARIABLE   
DESCRIPTION
GAPONLY 
Separation distance calculation flag: 
GAPONLY.EQ.0:  perform 
best-fit, 
separation 
distances  between  the  two  best-fitted  mesh 
parts. 
calculate 
GAPONLY.EQ.1:  no best-fit, just calculate separation distances 
between the two existing mesh parts. 
GAPONLY.EQ.2:  User is responsible to move the parts closer in 
distance  and  orientation,  in  situation  where 
target  and  source  are  not  similar  in  shape. 
Also  see  NSETS  and  NSETT  (recommended 
method). 
IFAST 
Computing performance optimization flag: 
IFSET 
IFAST.EQ.0:  no computing speed optimization. 
IFAST.EQ.1:  activate  computing  speed  optimization  (default),
and is recommended. 
See Table 12-21 for detailed speed performance data. 
Optional  flag  to  define  a  node  set  to  be  included  or  excluded  in
the source mesh file for best fitting.  The node set can be defined
in a file together with the source mesh.  A node set can be defined
using  LS-PrePost  via  menu  options  Model→CreEnt→Set 
Data→*SET_NODE→Cre. 
IFSET.EQ.0:  all nodes in the source mesh file will be best fitted.
IFSET.GT.0:  the input value is a node set ID; only the nodes in
VARIABLE   
DESCRIPTION
the set will be best fitted. 
IFSET.LT.0:  the  absolute  value  is  a  node  set  ID;  all  nodes
excluding  those  in  the  set  will  be  best  fitted.    See
Example 2. 
An  optional  node  set  ID  of  three  nodes  from  the  source  mesh.
The  nodes  should  be  selected  based  on  distinctive  geometry 
features, such as, the center of an arc, the center of a dart, or the
end  node  of  a  take-up  bead  . 
The three nodes must not be aligned in one straight line.  Define 
NSETS  if  the  orientation  of  the  source  mesh  deviates  from  the
target  is  large  (>~30  degrees  in  any  direction).    This  is  the
recommended method. 
An  optional  node  set  ID  from  the  target  mesh,  consists  of  the
corresponding  three  nodes  from  the  same  geometry  features  of
the  source  mesh.    The  three  nodes  should  be  input  in  the  same
order as those from the source mesh.  Approximate locations are
acceptable.  Define NSETT only if NSETS is defined.  See Example 
3 and Figure 12-22 for details.  This is the recommended method. 
Target mesh file in keyword format, where only *NODE and *EL-
EMENT_SHELL should be included.  The target mesh is typically
the  scanned  part  converted  from  the  STL  format  file.    STL  file 
format can be imported into  LS-PrePost via File→Import→STL File, 
then a keyword format mesh file can be saved. 
NSETS 
NSETT 
FILENAME 
Remarks: 
In springback prediction and compensation process simulation, there is always a need 
to assess the accuracy  of the springback prediction using physical white-light scanned 
parts.  Scanned parts are typically given in the STL format, which can be imported into 
LS-PrePost and written back out as a keyword mesh file. 
The converted scanned keyword file can be used as FILENAME as a target mesh in an 
input  file  .    The  predicted  springback  mesh  (source),  consisting  of 
*NODE, *ELEMENT_SHELL, *CONSTRAIN_ADAPTIVITY cards only, can be included 
in the input file using *INCLUDE.  The best-fit program uses an iterative least-squares 
method  to  minimize  the  separation  distances  between  the  two  parts,  eventually 
transforming  the  springback  mesh  (source)  into  the  position of  the  target  mesh  (scan).  
The  normal  distances  between  the  two  parts  are  calculated  after  the  best-fitting,  and 
stored as thickness values in a file bestfit.out, which is essentially a dynain file.
Both  positive  and  negative  distances  are  calculated  and  stored  as the  Thickness.    Color 
contours  of  the  normal  distances  between  the  two  parts  can  then  be  plotted  using 
COMP→Thickness.  Positive distance means the source mesh is above the target mesh in 
a  larger  coordinates,  and  negative  distance  is  below  the  target  mesh  in  a  smaller 
coordinates.  For areas where no corresponding meshes can be found between the two 
parts, the distances are set to nearly zero.  The fitting accuracy is within 0.02mm. 
To  reduce  the  computing  time  ,  the  scan  file  (STL)  mesh  can  be  coarsened  in  a  scan-
processing software from a typically very dense mesh to a more reasonably sized mesh.  
In  any  case,  the  coarser  mesh  should  be  selected  as  the  target  mesh  for  optimal 
computational speed. 
The fitted mesh bestfit.out and target mesh parts can both be imported into LS-PrePost.  
Using  the SPLANE  feature  in LS-PrePost,  multiple  sections  can  be  cut  on  both  parts  to 
assess springback deviations on a cut-section basis. 
It  is  suggested  that  the  orientation  of  the  included  file  (source)  should  be  within  30 
degrees in any direction of the target file.  In addition, the more rotations needed to re-
orient  the  include  file  to  align  with  the  target  file,  the  more  CPU  time  will  it  take  to 
complete the best fitting. 
In  case  the  source  mesh  orients  more  than  30  degrees  in  any  directions  of  the  target 
mesh,  NSETS  and  NSETT  can  be  used  to  initially  align  the  source  mesh  to  the  target 
mesh before a full best-fit is performed.  See Example 3 and Figure 12-22. 
Example 1 – fitting with all nodes from the included file: 
A  complete  input  example  is  provided  below  to  best  fit  a  source  mesh  part  spbk_
NoSS.k to the target mesh part scan.k.  NSKIP is set to “-5” and speed optimization is 
activated by setting IFAST to “1”. 
*KEYWORD 
*CONTROL_FORMING_BESTFIT 
$     IFIT     NSKIP   GAPONLY     IFAST     IFSET 
         1        -5         0         1         0 
scan.k 
*INCLUDE 
spbk_NoSS.k 
*END 
Example 2 – fitting with an excluded node set: 
From the previous example, the included source file spbk_NoSS.k now consists of node 
set  128.    The  node  set,  which  is  defined  in  the  file  spbk_NoSS.k,  which  may  feature 
geometry that are not a part of the target mesh, is being excluded (IFSET = -128) from
participating in the best fitting.  Alternatively, the unwanted nodes can be just deleted 
from the source file. 
*KEYWORD 
*CONTROL_FORMING_BESTFIT 
$     IFIT     NSKIP   GAPONLY     IFAST     IFSET 
         1        -5         0         1      -128 
scan.k 
*INCLUDE 
spbk_NoSS.k 
*END 
Example 3 – fitting with NSETS and NSETT (recommended): 
In  the  following  partial  keyword  example  (shown  in  Figure  12-22)  a  source  mesh 
sourcemesh.k is being best fitted to a target mesh targetmesh.k.  A node set with ID 1 
on  the  source  mesh  is  defined  consisting  of  nodes  1001  1002  and  1003  and  a 
corresponding node set with ID 2 on the target mesh is defined and consists of nodes 1, 
2 and 3. 
Node ID 1001 and 1 are both located at the center of a dart on the top surface of the hat-
shaped part.  Node ID 1002 and 2 are selected at the center of an arc of an cutout hole.  
Lastly,  node  ID  1003  and  3  are  at  the  center  of  a  tangent  line  of  a  radius.    With  the 
NSKIP  set  a  “-5”,  the  search  will  be  done  skipping  every  5  mm  of  distance.    In  this 
example, since the source and target meshes are exactly the same, the normal distance, 
as displayed by “thickness” is nearly zero everywhere. 
*CONTROL_FORMING_BESTFIT 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
$#    IFIT     NSKIP   GAPONLY     IFAST     IFSET     NSETS     NSETT 
         1        -5         0         1         0         1         2 
$# FILENAME 
targetmesh.k 
*INCLUDE 
sourcemesh.k 
*SET_NODE_LIST 
1 
1,2,3 
*SET_NODE_LIST 
2 
1001,1002,1003 
Revision information: 
This feature is available starting from LS-DYNA Revision 96427 double precision SMP.  
The  variable  IFSET  is  available  starting  from  Revision  96696.    The  variables  NSETS, 
NSETT  are  available  starting  from  Revision  99369.    The  VECTOR  option  is  available 
starting from Revision 112655.
Node 1
Node 3
Node 1002
Node 2
Node 1001
Node 1003
Source mesh
Target mesh
Best fit results of part separation
Contours of shell thickness
min=-9.39123e-06 at elem# 102
max=8.45032e-06 at elem# 149
Node 1: geometry feature 
such as the center of a dart 
is a preferred choice to be 
one of the three nodes.
Node 3: the 
center node of a 
tangent line may 
also be used. 
Node 2: the 
center of an arc 
of a hole can 
also be used to 
select one of the 
three nodes.
Part Separation
(mm)
8.450e-06
6.665e-06
4.881e-06
3.097e-06
1.313e-06
4.706e-07
-2.255e-06
-4.039e-06
-5.823e-06
-7.607e-06
-9.391e-06
Best fit results - color contour of part separation plotted with 
"thickness" from the output file "Bestfit.out" 
Figure 12-22.  Best fit of two meshes with orientations greater than 30 degrees
from each other.
*CONTROL_FORMING_INITIAL_THICKNESS 
Purpose:    This  keyword  is  used  to  specify  a  varying  thickness  field  in  a  specific 
direction  on  a  sheet  blank  (shell  elements  only)  as  a  result  of  a  metal  forming  process 
such  as  a  tailor-rolling,  to  be  used  for  additional  metal  forming  simulation.    Another 
related keyword includes *ELEMENT_SHELL_THICKNESS. 
  Card 1 
1 
2 
Variable 
PID 
LCID 
Type 
I 
I 
3 
X0 
F 
4 
Y0 
F 
5 
Z0 
F/I 
6 
VX 
F 
7 
VY 
F 
8 
VZ 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
PID 
LCID 
Part ID of the sheet blank to be defined with varying thickness, as
in *PART.  Currently only 1 PID is allowed. 
Load  curve  ID  defining  thickness  (Y-values)  vs.    distance  (X-
values) starting from position coordinates (X0, Y0, Z0) and in the
direction of a vector [VX, VY, VZ], as in *DEFINE_CURVE. 
X0, Y0, Z0 
Starting position coordinates. 
VX, VY, VZ 
Vector  components  defining  the  direction  of  the  distance  in  the
load curve. 
Background: 
Tailor-rolling  is  a  process  used  to  vary  the  thickness  of  the  blank.    A  judiciously 
designed  and  manufactured  tailor-rolled  blank  will  reduce  the  number  of  parts 
(reinforcements) involved in the stamping process, as well as the number tools needed 
to make them.  By reducing the number of spot welds, tailor-rolled pieces also possess 
superior structural integrity. 
Remarks: 
1.  Beyond  the  last  data  point  LS-DYNA  extrapolates  the  load  curve  specified  in 
LCID as being constant.
2.  This card overrides thicknesses set with the *SECTION_SHELL keyword. 
Application example: 
An  excerpt  from  an  input  deck  containing  a  characteristic  example  of  this  card’s 
application is given below.  In this example the blank is part ID 1.  The axis of the load 
curve starts at position (−295, −607, −43) and the direction along which the load curve 
sets the thickness is given by (524, 607, 0).  For each of the load curve’s abscissa values, 
𝑡, the corresponding geometrical coordinate is given by: 
𝒓 =
−295
−607
−43 ⎦
⎥⎤ +
⎢⎡
⎣
524
607
0 ⎦
⎥⎤ 𝑡 
⎢⎡
⎣
For negative values along the load curve, 𝑡 < 0, and values of 𝑡 > 101.0, the thickness is 
extrapolated as a constant value of 0.8, and 0.9, respectively. 
*CONTROL_FORMING_INITIAL_THICKNESS 
$      PID       LCID        X0        Y0        Z0        VX        VY        VZ 
         1       1012    -295.0    -607.0     -43.0     524.0     607.0       0.0 
*DEFINE_CURVE 
1012 
0.0, 0.8 
21.0, 0.9 
43.0, 1.0 
65.0, 1.1 
82.0, 1.0 
101.0, 0.9 
In Figure 12-23, a sheet blank is defined with a varying thickness across its surface in a 
vector  direction  pointed  from  the  start  to  end  point.    The  thickness  variation  vs.    the 
distance from starting point in section A-A is shown in Figure 12-24. 
Revision information: 
This feature is available in LS-DYNA starting in Revision 82990.
Contours of shell thickness
min=0.635661 at elem# 175119
max=1.29457 at elem# 177147
Ending point 
(distance=802mm)
Starting point 
(distance=0) 
Thickness (mm)
1.295
1.229
1.163
1.097
1.031
0.965
0.899
0.833
0.767
0.702
0.636
Figure 12-23.  Define a varying thickness field across the sheet blank. 
Input
Response
)
(
1.4
1.3
1.2
1.1
1.0
0.9
0.8
0.7
0.6
0.0
200.0
400.0
600.0
800.0
Distance Along Section (mm)
Figure 12-24.  Thickness variation across section A-A
*CONTROL_FORMING_MAXID 
Purpose:  This card sets the node and element ID numbers for an adaptive sheet blank.  
The  new  node  and  element  number  of  the  adaptive  mesh  will  start  at  the  values 
specified  on  this  card,  typically  greater  than  the  last  node  and  element  number  of  all 
tools  and  blanks  in  the  model.    This  keyword  is  often  used  in  multi-stage  sheet  metal 
forming simulation.  The *INCLUDE_AUTO_OFFSET keyword is related. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
MAXIDN  MAXIDE 
Type 
I 
I 
I 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION
PID 
Part ID of the sheet blank, as in *PART. 
Node ID number from which adaptive node ID numbers will be
created. 
Element  ID  number  from  which  adaptive  element  ID  numbers
will be created. 
MAXIDN 
MAXIDE 
Remarks: 
In a multi-stage automatic line die simulation the adaptivity feature may generate node 
and  element  IDs  that  collide  with  those  of  the  tools  used  in  the  later  stages  of  the 
process.    Before  the  calculation  begins,  the  set  of  IDs  used  by  the  tools  is  known.    By 
setting  MAXIDN  to  a  value  greater  than  the  largest  tool  node  ID  and  MAXIDE  to  a 
value  greater than  the  largest tool  element  ID,  it  is  guaranteed  that  refinement  during 
the early stages will not lead to conflicts with tool IDs in the later stages. 
The following example shows this feature applied in a 2D trimming simulation.  Nodes 
and  elements  ID  numbers  generated  from  an  adaptive  trim  simulation  will  be  larger 
than  the  specified  ID  numbers  of  5921980  and  8790292,  respectively,  for  a  sheet  blank 
with part ID of 4. 
*KEYWORD 
*INCLUDE_TRIM 
sim_trimming.dynain 
⋮
*CONTROL_ADAPTIVE_CURVE 
$    IDSET     ITYPE         N      SMIN 
   &blksid         2         2       0.6 
*CONTROL_CHECK_SHELL 
$     PSID    IFAUTO    CONVEX      ADPT    ARATIO     ANGLE      SMIN 
  &blksid1         1         1         1  0.250000150.000000  0.000000 
*INCLUDE 
EZtrim.k 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*DEFINE_CURVE_TRIM_NEW 
$#    tcid    tctype      tflg      tdir     tctol      toln    nseed1    nseed2 
     90914         2         0         1  1.250000  1.000000         0         0 
sim_trimming_trimline_01.igs 
*DEFINE_VECTOR 
$#     vid        xt        yt        zt        xh        yh        zh       cid 
         1     0.000     0.000     0.000     0.000     0.000  1.000000         0 
*CONTROL_FORMING_MAXID 
$      pid    maxidn    maxide 
         4   5921980   8790292 
*END 
Revision Information: 
This feature is available starting in LS-DYNA Revision 84159.
*CONTROL_FORMING_ONESTEP_{OPTION} 
Purpose:    This  keyword  activates  a  one-step  solution  using  the  total  strain  theory 
approximation  to  plasticity  (also  known  as  deformation  theory)  to  implement  an 
inverse  method.    Given  the  final  geometry,  the  one-step  method  uses  LS-DYNA’s 
implicit  statics  solver  to  compute  an  approximate  solution  for  (1)  the  stresses  and 
strains  in  the  formed  part,  (2)  the  thickness  of  the  formed  part,  and  (3)  the  size  of  the 
initial blank (unfolded flat blank).  This method is useful for estimating the initial blank 
size  with  attendant  material  costs,  and  for  augmenting  crashworthiness  models  to 
account  for  metal  forming  effects,  such  as  plastic  strains  and  blank  thickness  in  crash 
simulation. 
NOTE:  The  input  must  contain  only  one  “part”,  consisting 
entirely of shells, which is taken to be the final geometry. 
1.  This  “part”  may  involve  more  than  one  PID  to  accommo-
date welded blanks, 
2. 
3. 
it must be composed entirely of shells, and, 
its external boundary must consist of a single closed loop. 
Keywords associated with *CONTROL_FORMING_ONESTEP are: 
*CONTROL_FORMING_UNFLANGING 
*INTERFACE_BLANKSIZE_DEVELOPMENT. 
Available options include: 
<BLANK> 
AUTO_CONSTRAINT 
DRAWBEAD 
FRICTION 
TRIA 
QUAD 
QUAD2 (default) 
Summary of keyword options:
1.  The AUTO_CONSTRAINT option excludes rigid body motion from the implicit 
solution  by  automatically  adding  nodal  constraints.    A  deck  with  a  *CON-
TROL_FORMING_ONESTEP  card  should  contain  at  most  one  *CONTROL_-
FORMING_ONESTEP_AUTO_CONSTRIANT  card.    In  addition,  starting  from 
Revision  91229,  three  nodes  can  be  specified  on  the  final  part  to  position  the 
unfolded  blank  for  easier  blank  nesting,  and  for  blank  alignment  in  forming 
simulation. 
2.  The DRAWBEAD option is used to apply draw bead forces in addition to those 
provided  by  AUTOBD  field  in  Card  1.    A  deck  containing  a  *CONTROL_-
FORMING_ONESTEP card may contain as many *CONTROL_FORMING_ON-
ESTEP_DRAWBEAD cards as there are draw beads to be defined. 
3.  The FRICTION option applies friction along the edge of the part based on the 
binder tonnage input by the user in the DBTON field of card 1.  A deck contain-
ing  a  *CONTROL_FORMING_ONESTEP  card  may  contain  as  many  *CON-
TROL_FORMING_ONESTEP_FRICTION cards as there are friction node sets to 
be defined. 
4.  Originally all quadrilateral elements in the model were split into two triangular 
elements  internally  for  calculation.    This  original  formulation  is  set  as  option 
TRIA as of Revision 112682.  The option QUAD supports quadrilateral elements 
and  implements  some  improved  algorithm,  which  result  in  better  results.    In 
addition,  this  option  greatly  improves  calculation  speed  under  multiple  CPUs 
in SMP mode, and is available starting in Revision 112071.  The option QUAD2 
is  yet  another  improvement  over  the  option  QUAD  with  enhanced  element 
formulation,  which  further  improves  results  in  terms  of  thinning  and  plastic 
strain  with  slightly  longer  CPU  times.    Calculation  speed  comparisons  among 
the  three  options  can  be  found  in  Performance  among  options  TRIA,  QUAD.  
The  option QUAD2  is  set  as  a  default as  of Revision  112682  and  is  the  recom-
mended option. 
Card 1 for no option, <BLANK>. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OPTION  TSCLMAX  AUTOBD  TSCLMIN EPSMAX 
LCSDG 
DMGEXP 
Type 
Default 
I 
6 
F 
F 
F 
F 
I 
F 
1.0 
0.0 
1.0 
1.0 
none 
none
Card 1 for option AUTO_CONSTRAINT. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ICON 
NODE1 
NODE2 
NODE3 
Type 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
Card 1 for option DRAWBEAD. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NDSET 
LCID 
TH 
PERCNT 
Type 
I 
I 
F 
F 
Default 
none 
none 
0.0 
0.0 
Card 1 for option FRICTION. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NDSET 
BDTON 
FRICT 
Type 
I 
F 
F 
Default 
none 
0.0 
0.12
Card 2 for no option <BLANK>. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
  VARIABLE   
OPTION 
TSCLMAX 
FLATNAME 
A 
none 
DESCRIPTION
Options  to  invoke  the  one-step  solution  methods  which  account 
for undercut conditions in the formed part: 
EQ.6: One-step solution with unfolded blank (flat) provided by
LS-PrePost .  Card #2 is required. 
EQ.7: One-step  solution  with  blank  automatically  unfolded  in
LS-DYNA.    Card  #2  is  a  blank  line.    This  option  is  rec-
ommended. 
L.T.0: If a negative sign precedes any of the above OPTIONs, 
the stress and strain output in the file onestepresult will
be in a large format (E20.0), which leads to more accurate 
stress results. 
If  not  zero,  it  defines  a  thickness  scale  factor  limiting  the
maximum thickness in the part. 
For  example,  if  the  maximum  thickness  allowed  is  0.8mm  for  a
blank  with  initial  thickness  of  0.75mm  TSCLMAX  can  be  set  to
1.0667.  All thicknesses that are computed as more than 0.8mm in
the sheet blank will be reset to 0.8mm.  The scale factor is useful 
in  advance  feasibility  analysis  where  part  design  and  stamping
process have not been finalized and could potentially cause large
splits or severe wrinkles during unfolding, rendering the forming
results unusable for crash/safety simulation.
AUTOBD 
TSCLMIN 
EPSMAX 
LCSDG 
DMGEXP 
*CONTROL_FORMING_ONESTEP 
DESCRIPTION
Apply  a  fraction  of  a  fully  locked  bead  force  along  the  entire
periphery  of  the  blank. 
  The  fully  locked  bead  force  is
automatically  calculated  based  on  a  material  hardening  curve
input.    AUTOBD  can  be  increased  to  easily  introduce  more
thinning and effective plastic strain in the part. 
LT.0.0:  Turns off the “auto-bead” feature.  
EQ.0.0: Automatically applies 30% of fully locked force.  
GT.0.0: Fraction  input  will  be  used  to  scale  the  fully  locked
force. 
If  not  zero,  it  defines  a  thickness  scale  factor  limiting  the 
maximum thickness reduction. 
For  example,  if  the  minimum  thickness  allowed  is  0.6mm  for  a
blank with initial thickness of 0.75mm TSCLMIN can be set to 0.8.
All thicknesses that are computed as less than 0.6mm in the sheet
blank will be reset to 0.6mm.  The scale factor is useful in advance
feasibility analysis where part design and stamping process have
not  been  finalized  and  could  potentially  cause  large  splits  or
severe  wrinkles  during  unfolding,  rendering  the  forming  results
unusable for crash/safety simulation. 
If  not  zero,  it  defines  the  maximum  effective  plastic  strain
allowed.    All  computed  effective  plastic  strains  that  are  greater
than this value in the blank will be set to this value. 
Load  curve  ID  defining  equivalent  plastic  strain  to  failure  vs. 
stress triaxiality, see *MAT_ADD_EROSION. 
for 
see
Exponent 
*MAT_ADD_EROSION.    Damage  accumulation  is  written  as
history variable #6 in the file onestepresult. 
accumulation, 
nonlinear 
damage 
ICON 
Automatic  nodal  constraining  option  to  eliminate  the  rigid  body
motion: 
EQ.1: Apply.
VARIABLE   
NODE[1,2,3] 
NDSET 
LCID 
TH 
DESCRIPTION
Node  IDs  for  which  the  position  is  fixed  during  the  unfolding.
The position of these nodes in the calculated unfolded piece will
coincide  with  the  corresponding  nodes  in  the  input.    The
transformed and unfolded blank will be written in a keyword file
“repositioned.k”.    When  these  fields  are  undefined  the  orientation  of
the unfolded blank is arbitrary. 
Node  set  ID  along  the  periphery  of  the  part,  as  defined  by
keyword *SET_NODE_LIST. 
Load curve ID that defines the material hardening curve. 
Thickness of the unformed sheet blank. 
PERCNT 
Draw bead lock force fraction of the fully locked bead force. 
BDTON 
Binder tonnage used to calculate friction force. 
FRICT 
Coefficient of friction. 
FLATNAME 
File  name  of  the  initial  unfolded  blank  by  LS-PrePost  .  This is needed only for the OPTION = 6.  Leave a blank 
line for OPTION = 7. 
About One-Step forming solution: 
One-step solution employs the total strain (or deformation) theory of plasticity in place 
of  the  more  realistic  incremental  strain  (or  flow)  theory.    The  total  deformation  theory 
expresses stress as a function of total strain; whereas the incremental strain theory requires 
that  LS-DYNA  compute  a  stress  update  at  each  time  step  (strain  increment)  from  the 
deformation  that  occurred  during  that  time  step.    In  deformation  theory,  the  results, 
therefore, do not depend on strain path, forming history, or the details of the stamping 
process. 
When  this  card  is  included,  the  input  must  contain  the  final  geometry  from  which  LS-
DYNA calculates the initial flat state using the inverse method.  The one-step solution 
results can get close to the incremental results only when the forming process involves a 
linear  strain  path  for  which  the  deformation  is  either  monotonically  increasing  or 
decreasing.  In most cases total strain theory does not match incremental forming. 
Path independence leads to several key simplifications: 
1.  Binder and addendum geometry are not required.  There is no need to measure 
or model these geometries.
2.  The solution is independent of stamping die processes (including part tipping). 
3.  There  is  no  need  for  contact  treatment  since  there  are  no  tools  and  dies 
involved. 
The one-step solution is mostly used for advance formability studies in which the user 
needs  to  quickly  compare  a  wide  range  of  different  design  alternatives.    With  this 
method  the  user  can  evaluate  blank  size,  estimate  material  cost,  and  generate  a  first 
guess  for  blank  size  development  .  This method is also widely used to 
initialize forming stresses and strains in crash and occupant safety analysis. 
Input details: 
1.  Mesh.  In addition to the usual material and physical property definitions, this 
method requires that the final part be fully meshed using shell elements.  This 
mesh  must  satisfy  a  different  set  of  requirements  than  the  tooling  mesh.    In 
particular,  along  the  part  bend  radius,  there  is  no  need  to  build  six  elements 
along  the  arc  length  as  one  would  do  for  the  punch/die  radius;  two  elements 
may be enough.  A mesh consisting of uniformly distributed quadrilateral shell 
elements is ideal.  All elements in the mesh must also have normal consistency. 
With LS-PrePost 4.0, this kind of mesh can be generated using Mesh → AutoM → 
Size.    Since  this  method  uses  an  implicit  static  solution  scheme,  the  computa-
tional cost is controlled by the number of elements; element size has no effect.  
Furthermore, it is important to note that if one wants to obtain forming results 
that are closer to the incremental forming results, the part in the one-step input 
should  be  similar  in  size  to  the  final  formed  blank  shape  in  the  incremental 
forming (before trimming). 
2.  Holes.  Any trimmed-out holes can be filled (but not necessary).  The filling can 
be done semi-automatically using LS-PrePost 4.0 by selecting Mesh → EleGen → 
Shell → Shell by Fill_Holes → Auto Fill.  The filled area of the part can be saved in 
a different part, as multiple parts (PID) are allowed.  The forming results may 
depend on whether or not the holes are filled. 
3.  Unfolding.    For  OPTION =  6,  the  unfolded  blank  can  be  obtained  from  LS-
PrePost via EleTol → Morph →  Type = Mesh_Unfolding → Unfold.  The unfolded 
mesh  can  be  saved  as  a  keyword  file  and  used  as  input  .  With OPTION = 7, LS-DYNA unfolds the mesh itself. 
4.  Element Formulation.  Shell element of type 2 and 16 are supported.  Since this 
feature uses the implicit method, type 16 is more convergent, computationally 
efficient, and, therefore, strongly recommended.  Results are output on all inte-
gration points, as seen in the ELFORM and NIP variables in *SECTION_SHELL.
5.  Supported  Materials.    Currently,  *MAT_024,  and  *MAT_037  are  supported.  
The  user  must  provide  a  material  hardening  curve  either  in  the  LCSS  field  of 
*MAT_024 or in the HLCID field of *MAT_037.  For *MAT_024 tables are sup-
ported.  Future releases will add support for bilinear hardening with the ETAN 
feature.  Additionally, in *MAT_024, strain rate is ignored, even when the vari-
ables C, and P are set.  
6.  Boundary  Conditions.    The  primary  “boundary/loading  condition”  for  the 
one-step solution is the draw bead forces, which are set with the AUTOBD field 
or with the DRAWBEAD keyword option. 
a)  With the DRAWBEAD option, draw bead forces are applied on a user de-
fined node set .  A fraction of the full lock force, determined 
by  the  tensile  strength  and  sheet  thickness,  can  be  specified.    The  larger 
the  fraction,  the  less  the  metal  will  flow  into  the  die  resulting  in  more 
stretching and thinning. 
b)  Boundary conditions may also be set using the “Auto Beads” feature   with  which  draw  bead  forces  are  automatically  ap-
plied  to  all  nodes  along  the  part  boundary.    The  users  must  specify  the 
fraction of the fully locked bead force to be applied.  The default value of 
30% is sufficient for crash/occupant safety applications. 
The  last  important,  but  often  overlooked,  “boundary  condition”  is  the  part’s 
shape.  For example, an oil pan with a larger flange area will experience greater 
thinning  in  the  part  wall,  whereas  having  a  smaller  flange  area  will  have  the 
reverse effect.  To obtain results that are closer to the incremental strain theory, 
additional  materials  may  need  to  be  added  to  the  final  part  geometry  in  cases 
where  the  sheet  blank  is  not  “fully  developed,”  meaning  no  trimming  is  re-
quired to finish the part. 
7.  Friction.    Friction  effects  can  be  included  with  the  FRICTION  option.    The 
frictional force is based on an expected binder tonnage, and is a percentage of 
the input force.  Note that the binder tonnage value  is used exclu-
sively in calculating friction forces.  The binder tonnage is not actually applied 
on the binder as a boundary condition. 
8.  Rigid  Body  Motion.    LS-DYNA  will  automatically  add  nodal  constraints  to 
prevent rigid body motion when the AUTO_CONSTRAINT option is used and 
ICON is set to 1. 
9. 
Implicit  Solver  Options.    All  other  implicit  cards,  such  as  *CONTROL_IM-
*CONTROL_IM-
PLICIT_GENERAL, 
PLICIT_SOLVER, 
*CONTROL_IMPLICIT_-
TERMINATION,  etc.,  are  used  to  set  the  convergence  tolerance,  termination 
criterion,  etc.    The  two  most  important  variables  controlling  the  solution  con-
*CONTROL_IMPLICIT_SOLUTION, 
*CONTROL_IMPLICIT_AUTO,
vergence  are  DELTAU  from  *CONTROL_IMPLICIT_TERMINATION,  and 
DCTOL from *CONTROL_IMPLICIT_SOULTION.  Experience has shown that 
they  should  be  set  to  0.001  and  0.01,  respectively,  to  obtain  the  most  efficient 
solution with the best results.  Typically, four implicit steps are sufficient, and 
DT0  in  *CONTROL_IMPLICIT_GENERAL  and  ENDTIM  in  *CONTROL_TER-
MINATION  should  be  set  accordingly.    For  difficult  parts,  more  steps  maybe 
needed.    For  some  parts,  ILIMIT  in  *CONTROL_IMPLICIT_SOLUTION  may 
need to be set to “1” for the full Newton iteration. 
10.  Blank  Card.    Card  #2  for  no  option  <BLANK>  is  a  blank  card,  but  it  must  be 
present. 
Output: 
Results  are  stored  in  an  ASCII  file  named  “onestepresult”  using  the  dynain  format.  
This file contains the forming thickness, the stress and the strain fields on the final part.  
It  can  be  plotted  with  LS-PrePost.    One  quick  and  useful  LS-PrePost  plotting  feature  is 
the  “formability  contour  map”,  which  colors  the  model  to  highlight  various  forming 
characteristics  including  cracks,  severe  thinning,  wrinkles,  and  good  surfaces.    The 
formability map feature is located in Post → FLD → Formability. 
Additionally, the final estimated blank size in its initial, flat state is stored in the d3plot 
files.    The  d3plot  files  also  contain  intermediate  shapes  from  each  implicit  step.    The 
final blank mesh in its flat state can be written to a keyword file using LS-PrePost by the 
following steps: 
1.  Go to Post → Output → Keyword, 
2. 
check the box to include Element and Nodal Coordinates 
3.  move the animation bar to the last state, and, 
4. 
click on Curr and Write. 
In addition, blank outlines can be created by: 
1.  menu option Curve → Spline → From Mesh (Method), 
2. 
3. 
4. 
5. 
checking Piecewise → byPart, 
select the blank, 
click on Apply, and, 
finally,  save  the  curves  in  IGES  format  using  the  File  menu  at  the  upper  left 
corner.
Effect of TSCLMAX, TSCLMIN and EPSMAX: 
During the early stage of product design, the initial product specifications may lead to 
large strains and excessive thinning on the formed panel.  The ensuing one-step results 
would  not  be  suitable  to  be  used  in  a  crashworthiness  simulation.    However,  these 
kinds  of  forming  issues  are  certain  to  be  fixed  as  a  natural  part  of  the  design  and 
stamping  engineering process.    The  variables  TSCLMAX,  TSCLMIN  and  EPSMAX  are 
thus created to impose artificial limits on the thinning and plastic strains.  The variables 
provide  convenient  way  to  run  a  crash  simulation  with  approximate  and  reasonable 
forming effects before the design is finalized.  In the keyword below (which is a part of 
the firewall model with original thickness of 0.75mm), TSCLMIN and EPSMAX are set 
to 0.8 and 0.3, respectively. 
*CONTROL_FORMING_ONESTEP 
$   OPTION   TSCLMAX    AUTODB   TSCLMIN    EPSMAX      
         7                 0.5       0.8       0.3 
The  thickness  and  effective  plastic  strain  plots  for  the  firewall  model  are  shown  in 
Figures 12-29 and 12-30, respectively.  The minimum value in the thickness contour plot 
and maximum value in the plastic strain contour plot as shown in the upper left corner 
correspond to the values specified in TSCLMIN and EPSMAX, respectively. 
Similarly, TSCLMAX can be set to 1.0667 to limit the max thickening in the part to 
0.8mm: 
*CONTROL_FORMING_ONESTEP 
$   OPTION   TSCLMAX    AUTODB   TSCLMIN    EPSMAX      
         7    1.0667       0.5       0.8       0.3 
Reposition of unfolded flat blank: 
Often  times  the  input  to  one-step  simulation  is  the  final  product  part  in  the  car  axis 
system.    However,  after  the  simulation,  the  unfolded  flat  blank  will  be  in  a  different 
orientation and position, requiring users to manually reposition the blank to its desired 
orientation and position.  The variables NODE1, NODE2, NODE3 allow users to specify 
three  nodes  so  that  the  blank  is  transformed  onto  the  final  part  (the  input), 
superimposing  the  exact  same  three  nodes  in  both  parts.    In  an  example  shown  in 
Figure 12-32, the three nodes (Nodes 197, 210 and 171) are defined near the edges of two 
holes.    The  transformed  and  unfolded  flat  blank  (written  in  a  keyword  file  “reposi-
tioned.k”)  is  seen  superimposed  onto  the  final  part  according  to  the  three  nodes 
specified  (Figure  12-32  bottom).    If  these  nodes  are  not  defined,  the  simulation  will 
result  in  the  unfolded  flat  blank  in  a  state  shown  in Figure  12-32  (top),  undesirable  to 
most users.
Damage  accumulation  D 
*MAT_ADD_EROSION): 
*CONTROL_FORMING_ONESTEP 
is  calculated  based  on 
(refer 
to  manual  section 
DMGEXP
𝐷 = (
𝜀𝑝
𝜀𝑓
)
In  the  example  below,  load  curve  #500  provides  plastic  failure  strain  vs.    stress 
triaxiality  and  DMGEXP  is  assumed  to  be  1.254.    Since  the  damage  accumulation  is 
written  into  the  file  onestepresult  as  history  variable  #6,  the  variable  NEIP  in 
*DATABASE_EXTENT_BINARY should be set to at least ‘6”. 
*CONTROL_FORMING_ONESTEP 
$   OPTION              AUTODB   TSCLMIN    EPSMAX               LCSDG    DMGEXP 
         7                           0.8       0.3                 500     1.254 
*DEFINE_CURVE 
500 
-0.3,0.6 
-0.2,0.3 
0.0,0.2 
0.2,0.25 
0.4,0.46 
0.65,0.28 
0.9,0.18 
*DATABASE_EXTENT_BINARY 
$    NEIPH     NEIPS    MAXINT    STRFLG    SIGFLG    EPSFLG    RLTFLG    ENGFLG 
                   6         7         1 
$   CMPFLG    IEVERP    BEAMIP     DCOMP      SHGE     STSSZ 
                   1                   2 
The damage accumulation contour map from the file onestepresult can be plotted in LS-
PrePost. 
Effect of hole-cut on the forming results: 
In Figure 12-31, a thickness contour plot of a one-step calculation on the NCAC Taurus 
firewall model with its holes unfilled is shown.  The unfilled case will undergo slightly 
less thinning, since the holes will expand as material flows outward away from the hole.  
However, the thicknesses with holes filled are likely closer to reality, since the holes are 
mostly  filled  during  forming on  the  draw  panel  and  then  trimmed  off  afterwards  in  a 
trim process.  On the other hand, it is important to realize that not all the holes are filled 
in a draw panel.  Some holes are cut inside the part in the scrap area (but not all the way 
to  the  trim  line)  during  draw  process  to  allow  material  to  flow  into  areas  that  are 
difficult to form, so as to avoid splitting.
Application example: 
The  following  example  provides  a  partial  input  file  with  typical  control  cards.    It  will 
iterate  for  four  steps,  with  auto  beads  of  0%  lock  force  applied  around  the  part 
boundary, and with automatic nodal constraints. 
*CONTROL_TERMINATION 
$   ENDTIM 
       1.0 
*CONTROL_IMPLICIT_GENERAL 
$   IMFLAG       DT0 
          1     0.25 
*CONTROL_FORMING_ONESTEP 
$   OPTION              AUTODB      
         7 
*CONTROL_FORMING_ONESTEP_AUTO_CONSTRAINT 
$     ICON 
         1 
*CONTROL_IMPLICIT_TERMINATION 
$   DELTAU 
     0.001 
*CONTROL_IMPLICIT_SOLUTION 
$  NSLOLVR    ILIMIT    MAXREF     DCTOL     ECTOL 
         2        11      1200      0.01      1.00  
*CONTROL_IMPLICIT_SOLVER 
$   LSOLVR 
         5 
*CONTROL_IMPLICIT_AUTO 
$    IAUTO    ITEOPT    ITEWIN     DTMIN     DTMAX 
         0         0         0       0.0       0.0 
Additional cards below specify extra bead forces of 45% and 30% applied to node sets 
22 and 23 along the part periphery, respectively.  Also, the resulting friction forces with 
friction  coefficient  of  0.1  and  binder  tonnage  of  10000.0  N  used  for  friction  force  are 
applied on the same node sets. 
*CONTROL_FORMING_ONESTEP_DRAWBEAD 
$   NDSET      LCID        TH    PERCNT 
       22       200       1.6      0.45 
*CONTROL_FORMING_ONESTEP_DRAWBEAD 
       23       200       1.6      0.30 
*CONTROL_FORMING_ONESTEP_FRICTION 
$   NDSET     BDTON    FRICT 
       22   10000.0      0.1 
*CONTROL_FORMING_ONESTEP_FRICTION 
$   NDSET     BDTON    FRICT 
       23   10000.0      0.1 
The  one-step  forming  results  for  the  NCAC  Taurus  model’s  firewall  are  shown  in 
Figure 12-25.  The average element size across the blank is 8mm, and the trimmed part 
(with holes filled) consists of 15490 elements.  *MAT_24 was used with BH210 material 
properties.  On a 1 CPU Xeon E5520 Linux machine, it took 4 minutes to complete the 
run  with  a  total  of  four  steps.    The  thickness,  the  plastic  strain,  and  the  blank  size 
prediction were reasonable, as shown in Figures 12-26, 12-27 and 12-28.
Performance among options TRIA, QUAD and QUAD2: 
The  following  partial  keyword  input  is  an  example  of  using  the  option  QUAD.    Note 
the  draw  bead  force  parameter  AUTOBD  is  set  at  0.5.    Calculation  speed  comparison 
among options QUAD, QUAD2 and TRIA can be found in Table 12-1. 
*KEYWORD 
*include 
model.k 
*CONTROL_TERMINATION 
1.0 
*CONTROL_FORMING_ONESTEP_QUAD 
$#  option  maxthick    autobd   thinmin    epsmax 
         7                 0.5 
*CONTROL_FORMING_ONESTEP_AUTO_CONSTRAINT 
         1 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form    zero_v 
         1    0.2500         2         1         0         0         0         0 
*CONTROL_IMPLICIT_TERMINATION 
$#  deltau    delta1     ketol     ietol     tetol     nstep 
  0.001000     0.000     0.000     0.000     0.000         0 
*CONTROL_IMPLICIT_NONLINEAR 
$#  nsolvr    ilimit    maxref     dctol     ectol  not used     lstol      rssf 
        12        11       200  0.010000  0.100000     0.000     0.000     0.000 
$#   dnorm    diverg     istif   nlprint 
         0         0         0         2 
$#  arcctl    arcdir    arclen    arcmth    arcdmp 
         0         0     0.000         1         2 
*CONTROL_IMPLICIT_SOLVER 
5 
*PART 
   5000000   5000000   5000000 
*SECTION_SHELL 
   5000000        16        1.        5.        1. 
      0.72      0.72      0.72      0.72 
... 
Table 12-1 Calculation speed improvement with and without option _QUAD. 
Number 
of 
elements 
Calculation speed (D.P.  SMP Rev.112720, 8 CPUs) 
Option TRIA 
Option QUAD 
Option QUAD2 
A hat shape part 
71000 
21.0 min  
14.1 min  
16.6 min 
A  upper  dash 
panel 
61700 
24.5 min  
11.5 min  
17.2 min
Revision information: 
This  feature  is  available  starting  in  Revision  67778  SMP  and  double  precision  only.  
Over time, improvements are made to improve accuracy and speed up the calculation 
time; revision 110117 or later is recommended.  Historic revisions are listed as follows: 
1)Revision 73442: output of stress tensors 
2)Revision 75156: output of strain tensors. 
3)Revision 75854: variables THINPCT and EPXMAX are available. 
4)Revision 76709: holes are allowed. 
5)Revision 91229: variables NODE1, NODE2, NODE3 are available. 
6)Revision 108229: variables LCSDG and DMGEXP are available. 
7)Revision 111311: variable TSCLMAX is available. 
8)Revision 112071: option QUAD is available. 
9)Revision 112682: original formulation is designated as option TRIA.  A new option 
QUAD2 is activated. 
10)Revision  109680:  negative  value  of  OPTION  for  a  large  format  stress  and  strain 
output.
Figure  12-25.    A  trimmed  dash  panel  (firewall)  with  holes  auto-filled  using
LS-PrePost 4.0 (original model courtesy of NCAC Taurus crash model). 
Contours of shell thickness
min=0.478084, at elem# 3210698
max=1.10908, at elem# 3211511
Thickness (mm)
0.750
0.725
0.700
0.675
0.650
0.625
0.600
0.575
0.550
0.525
0.500
Figure 12-26.  Shell thickness prediction (t0 = 0.75mm). 
Contours of plastic strain
max ipt. value
min=0, at elem# 3008783
max=0.46, at elem# 3210698
Plastic strain
0.460
0.414
0.368
0.322
0.276
0.230
0.184
0.138
0.092
0.046
0.000
Figure 12-27.  Effective plastic strain Prediction.
Figure 12-28.  Initial blank size prediction (flat, not to scale). 
Contours of shell thickness
min=0.6, at elem# 3206053
max=0.923214, at elem# 3211511
Thickness (mm)
0.750
0.725
0.700
0.675
0.650
0.625
0.600
0.575
0.550
0.525
0.500
Figure 12-29.  Blank thickness prediction with TSCLMIN = 0.8.
Contours of plastic strain
max ipt. value
min=0, at elem# 3008801
max=0.3, at elem# 3204379
Plastic strain
0.300
0.270
0.240
0.210
0.180
0.150
0.120
0.090
0.060
0.030
0.000
Figure 12-30.  Effective plastic strain with EPSMAX = 0.3. 
Contours of shell thickness
min=0.538193, at elem# 3209452
max=0.974493, at elem# 3211511
Thickness (mm)
0.750
0.725
0.700
0.675
0.650
0.625
0.600
0.575
0.550
0.525
0.500
Figure 12-31.  Blank thickness with trimmed holes (t0 = 0.75mm).
Unfolded flat blank
Final part
Final part
Unfolded flat blank
N197
Figure 12-32.  An example of the results when using the NODE1, NODE2, and
NODE3  feature  (bottom)  and  without  using  the  feature  (top),  courtesy  of
Kaizenet Technologies Pvt Ltd, India. 
N210
N171
*CONTROL_FORMING_OUTPUT_{OPTION} 
Available options include: 
<BLANK> 
INTFOR 
Purpose:  This card defines the times at which states are written to the d3plot and intfor 
files based on the tooling’s distances from the home (final) position.  When the INTFOR 
option  is  set  this  keyword  card  controls  when  states  are  written  to  the  intfor  file, 
otherwise it controls the d3plot file.  This feature may be combined with parameterized 
input  and/or  automatic  positioning  of  the  stamping  tools  using  the  *CONTROL_-
FORMING_AUTOPOSITION_PARAMETER card. 
NOTE:  When this card is present no states are written except 
for those specified on this card.  This card supersedes 
the *DATABASE_BINARY_D3PLOT card. 
Forming Output Cards.  Repeat as many times as needed to define additional outputs 
in  separate  tooling  kinematics  curves.    The  next  keyword  (“*”)  card  terminates  the 
input. 
  Card 1 
1 
2 
3 
4 
5 
6 
Variable 
CID 
NOUT 
TBEG 
TEND 
Y1/LCID 
Y2/CIDT 
7 
Y3 
F 
8 
Y4 
F 
Type 
I 
Default 
none 
I 
0 
F 
F 
F/I 
F/I 
0.0 
none 
none 
none 
none 
none 
  VARIABLE   
CID 
DESCRIPTION
ID of a tooling kinematics curve.  This curve is integrated so that
the specified output distances can be mapped to times. 
For correct distance-to-time mapping CID must be applied to the 
tool  of  interest  using  a  *BOUNDARY_PRESCRIBED_MOTION_-
RIGID  card.    The  ordinate  scale  factor  SFO  in  the  *DEFINE_-
CURVE  is  supported  in  this  keyword  starting  from  Revision
82755.
)
(
-
0.0
-10
-20
-30
-40
-50
Y1 Y2 Y3
Y4
NOUT
&clstime
Punch displacement
NOUT
Y1
Y2
Y3
Y4
&endtime
0.0
0.002
0.004
0.006
0.008
0.01
0.012
Explicit time (sec.)
Figure 12-33.  An output example for closing and drawing.  See the example
provided at the end of this section. 
  VARIABLE   
NOUT 
TBEG 
TEND 
DESCRIPTION
Total  number  states  written  to  the  d3plot  or  intfor  databases  for 
the  tooling  kinematics  curve,  CID,  excluding  the  beginning  and
final states.  If NOUT is larger than the number of states specified
by either LCID or Yi fields (5 through 8), the remaining states are 
evenly distributed between TBEG and the time corresponding to
the biggest Yi from the home position, as shown in Figure 12-33. 
If  NOUT  is  left  as  blank  or  as  “0”,  the  total  number  of  output
states will be determined by either LCID or Yi’s. 
Start  time  of  the  curve.    This  time  should  be  consistent  with  the
BIRTH in *BOUNDARY_PRESCRIBED_MOTION_RIGID. 
End  time  of  the  curve.    This  time  should  be  consistent  with  the
DEATH  in  *BOUNDARY_PRESCRIBED_MOTION_RIGID.    This 
time is automatically reset backward removing any idling time if 
the tool finishes traveling early, so output distances can start from
the reset time.  A state is written at TEND.
Y1/LCID, 
Y2, Y3, Y4 
Y2/CIDT 
*CONTROL_FORMING_OUTPUT 
DESCRIPTION
Y1/LCID.GT.0: All  four  variables  (Y1,  Y2,  Y3,  Y4)  are  taken  to
be  the  distances  from  the  punch  home,  where
d3plot files will be output. 
Y1/LCID.LT.0:  The  absolute  value  of  Y1/LCID  (must  be  an
integer)  is  taken  as  a  load  curve  ID  .    Only  the  abscissas  in  the  load 
curve,  which  are  the  distances  to  punch  home,
are used.  These distances specify the states that
are written to the d3plot files.  Ordinates of the 
curve  are  ignored.    This  case  accommodates
more states than is possible with the four varia-
  Furthermore,  when 
bles  Y1,  Y2,  Y3,  Y4. 
Y1/LCID < 0, Y2, Y3, and Y4 are ignored. 
Available  starting  from  Revision  112604,  the
output will be skipped for any negative abscissa
in the load curve.  Note all abscissas being nega-
tive are not allowed. 
Y2/CIDT.GT.0: The  input  is  taken  as  the  distance  from  the
punch home, where a d3plot file will be output.
Y2/CIDT.LT.0:  The  absolute  value  of  Y2/CIDT  (must  be  an
integer)  is  taken  as  a  load  curve  ID  .    Only  the  abscissas  in  the  load 
curve, which are the simulation times, are used. 
These times specify the states that are written to
the  d3plot  files.    Ordinates  of  the  curve  are  ig-
nored.    Note  this  time-dependent  load  curve 
will output additional d3plot files on top of the 
d3plot files already written in case Y1/LCID < 0 
(if specified).  Furthermore, when Y2/CIDT < 0,
Y3 and Y4 are ignored.  See an example for us-
age. 
Motivation: 
In  stamping  simulations  not  all  time  steps  are  of  equal  interest  to  the  analyst.    This 
feature  allows  the  user  to  save  special  states,  usually  those  for  which  wrinkling  and 
thinning conditions arise as the punch approaches its home position.
This feature is available in Application eZ-Setup in LS-PrePost4.0 (http://ftp.lstc.com/-
anonymous/outgoing/lsprepost/4.0/metalforming/). 
Remarks: 
1.  Keywords  *DATABASE_BINARY_D3PLOT  and  *DATABASE_BINARY_INT-
FOR are not required (ignored if present) to output D3PLOT and INTFOR files 
when this keyword is present; 
2. 
3. 
*CONTROL_FORMING_OUTPUT  and  *CONTROL_FORMING_OUTPUT_-
INTFOR can share the same CIDs; 
If columns 5 through 8 are left blank, output (NOUT) will be evenly distributed 
through the travel; 
4.  The variable NOUT has priority over the number of points on the LCID; 
5.  Distances  input  (in  LCID)  that  are  greater  than  the  actual  tool  travel  will  be 
ignored; 
6.  Distance  input  (in  LCID)  does  not  necessarily  have  to  be  in  a  descending  or 
ascending order. 
Applicability: 
This  keyword  is  applicable  to  the  parameter  VAD  of  “0”  (velocity)  in  *BOUNDARY_-
PRESCRIBED_MOTION_RIGID,  and  for  explicit  dynamics  only.    Tooling  kinematics 
profiles  of  various  trapezoids  (including  right  trapezoid)  are  all  supported.    Local 
coordinate systems are supported.
Y1 Y2 Y3 Y4
&vcls
0.0
&tramp
&clstime
Explicit time
Figure  12-34.    Specifying  d3plot/intfor  output  at  specific  distances  to  punch
home. 
Application example for an air draw: 
In a keyword example below (air draw, referring to Figures 12-33 and 12-35), a total of 
five states will be output during a binder closing.  The kinematics are specified by the 
curve of ID 1113, which defines tooling kinematics starting time 0.0 and ending at time 
&clstime. 
Curve 1113 is used to associate the specified distances to the appropriate time step.  In 
this example NOUT is set to 5.  Of these five outputs states the last four will be output 
at  upper  die  distance  to  closing  of  3.0,  2.0,  1.0,  and  0.5  mm  according  to  the  values 
specified in the Y1, Y2, Y3, and Y4 fields. 
Similarly,  a  total  of  eight  states  will  be  written  to  the  d3plot  file  made  during  draw 
forming  according  curve  ID  1115,  which  defines  tooling  kinematics  starting  at  time 
&clstime, and ending at time &endtime.  Of the eight states the last four will be output at 
punch distance to draw home of 6.0, 4.0, 3.0, and 1.0 mm; the remaining four outputs will 
be evenly distributed between starting punch distance to home and punch distance of 6.0mm to 
home. 
Likewise,  for  intfor,  15  states  will  be  written  before  closing  and  18  states  after  the 
closing.  The d3plot and intfor files will always be output for the first and last states as a 
default; and at where the two curves meet at &clstime, only one d3plot and intfor will be 
output. 
To output intfor, “S=filename” needs to be specified on the command line, and SPR and 
MPR need to be set to “1” on the *CONTACT_… cards. 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*CONTROL_FORMING_OUTPUT 
$      CID      NOUT      TBEG      TEND        y1        y2        y3        y4
1113         5            &clstime       3.0       2.0       1.0       0.5 
      1115         8  &clstime  &endtime       6.0       4.0       3.0       1.0 
*CONTROL_FORMING_OUTPUT_INTFOR 
$      CID      NOUT      TBEG      TEND        y1        y2        y3        y4 
      1113        15            &clstime       3.5       2.1       1.3       0.7 
      1115        18  &clstime  &endtime      16.0       4.4       2.1       1.3 
*BOUNDARY_PRESCRIBED_MOTION_RIGID 
$   typeID       DOF       VAD      LCID        SF       VID     DEATH     BIRTH 
&udiepid           3         0      1113      -1.0         0  &clstime       0.0 
&bindpid           3         0      1114       1.0         0  &clstime       0.0 
&udiepid           3         0      1115      -1.0         0  &endtime  &clstime 
&bindpid           3         0      1115      -1.0         0  &endtime  &clstime 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*DEFINE_CURVE 
1113 
0.0,0.0 
&clsramp,&vcls 
&clstime,0.0 
*DEFINE_CURVE 
1114 
0.0,0.0 
10.0,0.0 
*DEFINE_CURVE 
1115 
0.0,0.0 
&drwramp,&vdraw 
&drwtime,&vdraw 
The keyword example below illustrates the use of load curves 3213 and 3124 to specify 
the  states  written  to  the  d3plot  and  intfor  files  respectively.    In  addition  to  the  eight 
states  specified  by  curve  3213,  five  additional  outputs  will  be  generated.   Similarly,  in 
addition  to  the  10  intfor  states  defined  by  curve  3214,  eight  additional  states  will  be 
output. 
*CONTROL_FORMING_OUTPUT 
$      CID      NOUT      TBEG      TEND        y1        y2        y3        y4 
      1113        13            &clstime     -3213 
*CONTROL_FORMING_OUTPUT_INTFOR 
$      CID      NOUT      TBEG      TEND        y1        y2        y3        y4 
      1113        18            &clstime     -3214 
*DEFINE_CURVE 
3213 
88.0 
63.0 
42.0 
21.5 
9.8 
5.2 
3.1 
1.0 
*DEFINE_CURVE 
3214 
74.0 
68.0 
53.0 
32.0 
25.5 
7.8 
4.2 
2.1 
1.4 
0.7
Application example for a multiple flanging process: 
Referring to Figure 12-36 and a partial keyword example listed below, flanging steels #1 
through #4 are defined as parameters &flg1pid through &flg4pid, respectively, which are 
moving  in  their  own  local  coordinate  systems.    The  termination  time  &endtime  is 
defined as pad closing time &clstime plus the maximum travel time of all four flanging 
steels.  A total of ten d3plot states and ten intfor states are defined for each flanging steel 
using  curve  IDs  980  and  981,  respectively.    Curve  values  outside  of  the  last  10  states 
(distances) are ignored; and reversed points are automatically adjusted.   
In Figure 12-37, locations of d3plot states are indicated by “x” markers for each flanging 
steel  move.    Note  that  for  flanging  steels  with  longer  travel  distances,  there  may  be 
additional  d3plot  states  between  the  defined  points,  controlled  by  distance  output 
defined for other flanging steels with shorter travels.  The total number of d3plot (and 
intfor)  states  is  the  sum  of  all  nout  defined  for  each  flanging  steel  so  care  should  be 
taken to limit the total d3plot (and intfor) states, especially if large number of flanging 
steels are present. 
*KEYWORD 
$  -------------------------closing 
*BOUNDARY_PRESCRIBED_MOTION_RIGID 
$   typeID       DOF       VAD      LCID        SF       VID     DEATH     BIRTH 
    &upid1         3         0      1113  &padvdir         0  &clstime 
*BOUNDARY_PRESCRIBED_MOTION_RIGID_local 
  &flg1pid         3         0      1114       1.0         0  &clstime 
  &flg2pid         3         0      1114       1.0         0  &clstime 
  &flg3pid         3         0      1114       1.0         0  &clstime 
  &flg4pid         3         0      1114       1.0         0  &clstime 
$  -------------------------flanging 
*BOUNDARY_PRESCRIBED_MOTION_RIGID 
$   typeID       DOF       VAD      LCID        SF       VID     DEATH     BIRTH 
    &upid1         3         0      1115  &padvdir         0            &clstime 
*BOUNDARY_PRESCRIBED_MOTION_RIGID_local 
  &flg1pid         3         0      1116       1.0         0            &clstime 
  &flg2pid         3         0      1117       1.0         0            &clstime 
  &flg3pid         3         0      1118       1.0         0            &clstime 
  &flg4pid         3         0      1119       1.0         0            &clstime 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*DEFINE_CURVE 
      1116 
                 0.0                 0.0 
             &tdrwup               &vdrw 
             &tdown1               &vdrw 
            &drw1tim                 0.0 
             1.0E+20                 0.0 
*DEFINE_CURVE 
      1117 
                 0.0                 0.0 
             &tdrwup               &vdrw 
             &tdown2               &vdrw 
            &drw2tim                 0.0 
             1.0E+20                 0.0 
*DEFINE_CURVE 
      1118 
                 0.0                 0.0 
             &tdrwup               &vdrw 
             &tdown3               &vdrw 
            &drw3tim                 0.0
1.0E+20                 0.0 
*DEFINE_CURVE 
      1119 
                 0.0                 0.0 
             &tdrwup               &vdrw 
             &tdown4               &vdrw 
            &drw4tim                 0.0 
             1.0E+20                 0.0 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*DEFINE_CURVE 
980 
60.0 
55.0 
42.0 
40.0 
38.0 
31.0 
23.0 
19.0 
15.0 
13.0 
13.5 
5.0 
3.0 
2.0 
2.5 
1.0 
*DEFINE_CURVE 
981 
23.0 
19.0 
15.0 
13.0 
13.5 
  ⋮  
*CONTROL_FORMING_OUTPUT 
$ -------1---------2---------3---------4---------5---------6---------7---------8 
$      CID      NOUT      TBEG      TEND   Y1/LCID 
      1116        10  &clstime  &endtime      -980 
      1117        10  &clstime  &endtime      -980 
      1118        10  &clstime  &endtime      -980 
      1119        10  &clstime  &endtime      -980 
*CONTROL_FORMING_OUTPUT_INTFOR 
$ -------1---------2---------3---------4---------5---------6---------7---------8 
$      CID      NOUT      TBEG      TEND   Y1/LCID 
      1116        10  &clstime  &endtime      -981 
      1117        10  &clstime  &endtime      -981 
      1118        10  &clstime  &endtime      -981 
      1119        10  &clstime  &endtime      -981 
        ⋮          ⋮       ⋮         ⋮            ⋮ 
An example of using CIDT: 
The example below shows in addition to the 7 states output based on various distances 
from  punch  home,  defined  by  load  curve  980,  4  more  states  are  output  based  on 
simulation time, defined by load curve 999. 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*DEFINE_CURVE 
999 
1.0e-03 
2.0e-03
3.0e-03 
4.0e-03 
*DEFINE_CURVE 
980 
13.5,0.0 
13.0,0.0 
5.0,0.0 
3.0,0.0 
2.5,0.0 
2.0,0.0 
1.0,0.0 
*CONTROL_FORMING_OUTPUT 
$ -------1---------2---------3---------4---------5---------6---------7---------8 
$      CID      NOUT      TBEG      TEND   Y1/LCID   Y2/CIDT 
      1116         0  &clstime  &endtime      -980     -999 
      1117         0  &clstime  &endtime      -980     -999 
      1118         0  &clstime  &endtime      -980     -999 
      1119         0  &clstime  &endtime      -980     -999 
Revision information: 
This  feature  is  available  starting  from  LS-DYNA  Revision  74957.    Other  options’ 
availabilities are as follows: 
7.  Y1/LCID is available from Revision 81403. 
8.  The scale factor SFO for ordinate values in *DEFINE_CURVE is supported from 
Revision 82755. 
9.  Output for multiple tools is available from Revision 83090. 
10.  Support for arbitrary BIRTH and DEATH in *BOUNDARY_PRESCRIBED_MO-
TION_RIGID is available from Revision 83090. 
11.  The INTFOR option is available from Revision 83757. 
12.  Y2/CIDT is available from Revision 110091. 
13.  Negative abscissa in the LCID is available starting from Revision 112604.
Time = 0.0051966
Time = 0.01366
Binder closing
Punch home
Figure 12-35.  An air draw example with closing and drawing. 
Flanging steel #4
Flanging steel #3 (hidden behind)
Flanging steel #2
Upper pressure pad
Flanging steel #1
Figure 12-36.  An example of multiple flanging process. 
Distance to home - &flg4pid:
23.0
15.0
13.0
19.0
13.5
5.0
3.0
2.5
2.0
1.0
&flg1pid
&flg2pid
&flg3pid
&flg4pid
)
(
30
25
20
15
10
0.0
0.002
0.004
0.006
0.008
&endtime
Explicit time (sec.)
  Figure 12-37.  D3PLOT/INTFOR output in case of multiple flanging process.
*CONTROL_FORMING_PARAMETER_READ 
Purpose:    This  feature  allows  for  reading  of  a  numerical  number  from  an  existing  file 
and  store  in  a  defined  parameter.    The  parameter  can  be  used  and  referred  in  the 
current simulation.  The file to be read may be a result from a previous simulation.  The 
file may also simply contain a list of numbers defined beforehand and to be used for the 
current simulation. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
FILENAME 
C 
Parameter Cards.  Include one card for each parameter.  The next “*” card terminates 
the input. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  PARNAME  METHOD 
LINE # 
BEGIN 
END 
Type 
C 
Default 
none 
I 
0 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
FILENAME 
Name of the file to be read. 
PARNAME 
Parameter name.  Maximum character length: 7. 
METHOD 
Read instruction: 
EQ.1: read,  follow  definition  by  LINE#,  BEGIN  and  END
definition 
LINE # 
Line number in the file. 
BEGIN 
Beginning column number in the line number defined above. 
END 
Ending column number in the line number defined above.
Remarks: 
1.  Keyword input order is sensitive.  Recommended order is to define variables in 
*PARAMETER first, followed with this keyword, using the defined variables. 
2.  Multiple  variables  can  be  defined  with  one  such  keyword,  with  the  file  name 
needed to be defined only once.  If there are variables located in multiple files, 
the keyword needs to be repeated for each file. 
3.  An example provided below shows that multiple PIDs for individual tools and 
blank  are  defined  in  files  “data.k”  and  “data1.k”.    In  the  main  input  file 
“sim.dyn” used for LS-DYNA execution, variables (integer) are first initialized 
for PIDS of all tools and blank with *PARAMETER.  These variables are updat-
ed  with  integers  read  from  files  “data.k”  and  “data1.k”  from  respective  line 
number  and  column  number  through  the  use  of  this  keyword.    In  the  *SET_-
PART_LIST definition, these PIDs are used to define the part set. 
Below is file “data.k”, to be read into “sim.dyn:: 
$$$$$$$$$$$$$$$$$$$$$$$$$ 
$$$ define PIDs 
$$$$$$$$$$$$$$$$$$$$$$$$$ 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- 
upper die  pid:              3 
lower post pid:              2 
Below is file “data1.k”, also to be read into “sim.dyn”: 
$$$$$$$$$$$$$$$$$$$$$$$$$ 
$$$$$$$$$$$$$$$$$$$$$$$$$ 
$$$$$$$$$$$$$$$$$$$$$$$$$ 
$$$ define PIDs 
$$$$$$$$$$$$$$$$$$$$$$$$$ 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- 
lower binder pid:            4 
blank pid:                   1 
Below is partial input for the main input file “sim.dyn”: 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- 
*INCLUDE 
blank.k 
*INCLUDE 
tool.k 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- 
*PARAMETER 
Iblankp,0 
Iupdiep,0 
Ipunchp,0 
Ilbindp,0 
Rblankmv,0.0 
Rpunchmv,0.0 
Rupdiemv,0.0 
Rbindmv,0.0 
Rbthick,1.6 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- 
*CONTROL_FORMING_PARAMETER_READ 
data.k 
updiep,1,5,30,30 
punchp,1,6,30,30 
*CONTROL_FORMING_PARAMETER_READ
data1.k 
lbindp,1,7,30,30 
blankp,1,8,30,30 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- 
*SET_PART_LIST 
1 
&blankp 
*SET_PART_LIST 
2 
&punchp 
*SET_PART_LIST 
3 
&updiep 
*SET_PART_LIST 
4 
&lbindp 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- 
*CONTROL_FORMING_AUTOPOSITION_PARAMETER_SET 
$#    psid       cid       dir     mpsid  position   premove    thick parname 
         1         0         3         2         1     0.000  &bthick blankmv 
         3         0         3         1         1     0.000          updiemv 
         4         0         3         1        -1     0.000           bindmv  
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- 
*PART_MOVE 
$pid,xmov,ymov,zmov,cid,ifset 
1,0.0,0.0,&blankmv,,1 
3,0.0,0.0,&updiemv,,1 
4,0.0,0.0,&bindmv,,1 
4.  This feature is available in LS-DYNA R5 Revision 55035 and later releases.
*CONTROL_FORMING_POSITION 
Purpose:    This  keyword  allows  user  to  position  tools  and  a  blank  in  setting  up  a 
stamping process simulation.  All tools must be pre-positioned at their home positions.  
For tools that are positioned above the sheet blank (or below the blank) and ready for 
forming,  *CONTROL_FORMING_TRAVEL  should  be  used.    This  keyword  is  used 
together  with  *CONTROL_FORMING_USER.    One  *CONTROL_FORMING_POSI-
TION card may be needed for each part. 
NOTE:  This  option  has  been  deprecated  in  favor  of  *CON-
TROL_FORMING_AUTOPOSITION_PARAME-
TER). 
Positioning Cards.  For each part to be positioned include an additional card.  The next 
“*” card terminates the input. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
PREMOVE  TARGET 
Type 
I 
F 
Default 
none 
none 
I 
I 
  VARIABLE   
DESCRIPTION
PID 
Part ID of a tool to be moved, as in *PART 
The  distance  to  pre-move  the  tool,  in  the  reverse  direction  of 
forming.  
Target tool PID, as in *PART.  The tool (PID) will be moved in the
reverse  direction  of  the  forming  and  positioned  to  clear  the
interference  with  the  blank,  then  traveled  to  its  home  position
with a distance GAP (*CONTROL_FORMING_USER) away from 
the TARGET tool to complete the forming. 
PREMOV 
TARGET 
Remarks: 
When  this  keyword  is  used,  all  stamping  tools  must  be  in  their  respective  home 
positions, which is also the position of each tool at its maximum stroke.  From the home 
position each tool will be moved to its start position, clearing interference between the 
blank  and  tool  yet  maintaining  the  minimum  separation  needed  to  avoid  initial
penetration.  Currently the tools can only be moved and travels in the direction of the 
global Z-axis. 
A  partial  keyword  example  is  provided  in  manual  pages  under  *CONTROL_FORM-
ING_USER. 
Revision information: 
This feature is available starting in Revision 24641.
*CONTROL_FORMING_PRE_BENDING 
Purpose:  This keyword allows for a pre-bending of an initially flat sheet metal blank, 
typically used in controlling its gravity loaded shape during sheet metal forming.  
  Card 1 
1 
2 
Variable 
PSET 
RADIUS 
Type 
I 
F 
3 
VX 
F 
4 
VY 
F 
5 
VZ 
F 
6 
XC 
F 
7 
YC 
F 
8 
ZC 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
PSET 
Part set ID to be included in the pre-bending. 
RADIUS 
Radius of the pre-bending. 
GT.0.0: bending  center  is  on  the  same  side  as  the  element
normals 
LT.0.0:  bending  center  is  on  the  reverse  side  of  the  element 
normals. 
See figure below for more information.  
VX, VY, VZ 
XC, YC, ZC 
Vector  components  of  an  axis  about  which  the  flat  blank  will  be
bent. 
X,  Y,  Z  coordinates  of  the  center  of  most-bent  location.    If 
undefined, center of gravity of the blank will be used as a default.
About pre-bending for gravity: 
In some situation, a flat blank upon gravity loading will result in a “concave” shape in a 
die.    This  mostly  happens  in  cases  where  there  is  little  or  no  punch  support  in  the 
middle of the die cavity and in large stamping dies.  Although the gravity loaded blank 
shape  is  correct  the  end  result  is  undesirable.    In  these  conditions,  buckles  may  result 
during the ensuing  closing and forming simulation.  In reality, a true flat blank rarely 
exists.  Typically, the blank is either manipulated (shaking or bending) by die makers in 
the tryout stage, or by suction cups in a stamping press, to get an initial convex shape 
prior to the binder closing and punch forming.  This keyword allows this bending to be 
performed.
*CONTROL_FORMING_PRE_BENDING 
A  partial  keyword  example  (NUMISHEET2022  fender  outer)  is  provided  below,  where 
blank part set ID variable &BLKSID is defined previously, is to be bent in a radius value 
of  -10000.0mm,  with  the  bending  axis  of  Z,  located  on  the  reverse  side  of  the  blank 
positive normal (Figure 12-38).  The bending is off gravity center at x = 234.0, y = 161.0, 
z = 81.6  (to the  right  along  positive X-axis).    Only  a  slight  pre-bending  on  the  blank  is 
needed to ensure a convex gravity-loaded shape.  
*KEYWORD 
⋮  
*CONTROL_IMPLICIT_FORMING 
1 
*CONTROL_FORMING_PRE_BENDING 
$     PSET    RADIUS        VX        VY        VZ        XC        YC        ZC 
   &BLKSID   -10000.      0.00      0.00      1.0    234.000   161.000     81.60 
... 
*END 
In  Figures  12-39,  initial  blank  shape  without  pre-bending  is  shown.    Without  pre-
bending,  the  gravity  loaded  blank  sags  in  the  middle  of  the  die  cavity,  Figure  12-40, 
which is likely unrealistic, and would lead to predictions of surface quality issues.  With 
pre-bending  applied,  Figure  12-41,  blank  bends  slight  and  in  convex  shape  before 
loading.  This shape results in an overall convex shape after gravity completes loading 
(Figure  12-42),  leading  to  a  much  shorter  binder  closing  distance,  and  a  more  realistic 
surface quality assessment. 
Revision information: 
This feature is available in double precision LS-DYNA Revision 66094 and later releases.  
It  is  also  available  in  LS-PrePost4.0  eZ-Setup  for  metal  forming  application  (http://-
ftp.lstc.com/anonymous/outgoing/lsprepost/4.0/metalforming/).
Sheet blank 
normal direction 
Bending axis
Figure 12-38.  Negative “R” puts center of bending on the opposite side of the
positive blank normal. 
Sheet blank
Lower binder
Lower punch
Figure 12-39.  Initial model before auto-positioning. 
Blank sags in 
the die cavity
Gravity loaded 
sheet blank
Figure 12-40.  Gravity loaded blank without using this keyword.
Sheet blank pre-bent with R=10000 mm
Figure 12-41.  Pre-bending using this keyword (1st state of D3plots). 
Gravity loaded on 
pre-bensheet blank 
 Figure 12-42.  Gravity loaded shape (last state of D3plots) with convex shape.
*CONTROL_FORMING_PROJECTION 
Purpose:    To  remove  initial  penetrations  between  the  blank  and  the  tooling  (shell 
elements  only)  by  projecting  the  penetrated  blank  (slave)  nodes  along  a  normal 
direction  to  the  surface  of  the  blank  with  the  specified  gap  between  the  node  and  the 
tooling surface.  This is useful for line die simulation of the previously formed panel to 
reduce tool travel therefore saving simulation time. 
Define Projection Card.  This card may not be repeated. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IDPS 
IDPM 
GAP 
NRSST 
NRMST 
Type 
I 
I 
F 
I 
I 
Default 
  VARIABLE   
DESCRIPTION
IDPS 
IDPM 
GAP 
Part ID of the blank (slave side). 
Part ID for the tool (master side). 
A distance, which defines the minimum gap required. 
NRSST 
Normal direction of the blank: 
EQ.0: the normal to the surface of the blank is pointing towards
the tool, 
EQ.1: the  normal  to  the  surface  of  the  blank  is  pointing  away
from the tool. 
NRMST 
Normal direction of the tool: 
EQ.0: the normal to the surface of the tool is pointing towards
the blank, 
EQ.1: the  normal  to  the  surface  of  the  tool  is  pointing  away
from blank. 
Remarks: 
This feature requires consistent normal vectors for both the rigid tooling surface and the 
blank surface.
*CONTROL_FORMING_PROJECTION 
This feature is available starting in Revision 25588.
*CONTROL_FORMING_REMOVE_ADAPTIVE_CONSTRAINTS 
Purpose:    This  keyword  converts  an  adaptive  mesh  into  a  fully  connected  mesh.  
Adaptive  constraints  are  removed  and  triangular  elements  are  used  to  connect  the 
mesh. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
Type 
Default 
I 
0 
  VARIABLE   
PID 
Remarks: 
DESCRIPTION
Part  ID  (as  in  *PART)  of  the  part  whose  adaptive  mesh
constraints  is  to  be  removed  and  its  mesh  converted  into 
connected meshes. 
In  some  application  in  sheet  metal  forming, such  as  stoning  or  spirngback  simulation, 
adaptive  refinement  on  the  sheet  blank  may  affect  the  accuracy  of  the  calculation.    To 
avoid this problem, non-adapted mesh is required.  However, adaptively refined mesh 
has  the  optimal  mesh  density  that  is  tailored  to  the  tooling  geometry;  the  resulting 
mesh, in its initial shape, either flat or deformed, has fewer elements (than a blank with 
non-adapted  and  uniformly-sized  elements)  and  thus  is  the  most  efficient  for 
simulation.  If the parameter IOFLAG in *CONTROL_ADAPTIVE is turned on, such a 
mesh  adapt.msh  will  be  generated  at  the  end  of  each  simulation,  with  its  shape 
conforming to the initial input blank shape. 
This  keyword  takes  the  adapted  mesh,  removes  the  adaptive  constraints,  and  use 
triangular elements to connect the otherwise disconnected mesh.  The resulting mesh is 
a  fully  connected  mesh,  with  the  optimal  mesh  density,  to  be  used  to  rerun  the 
simulation (without mesh adaptivity) for a better accuracy. 
Note  that  the  original  adapt.msh  file  from  a  LS-DYNA  run  will  include  not  only  the 
blank but the tooling mesh as well.  In order to be used for this keyword, the original 
file  can  be  read  into  LS-PrePost,  with  blank  shown  in  active  display  only,  and  menu 
option  File  →  Save  As  →  Save  Active  Keyword  As  can  be  used  to  write  out  the  adapted 
blank mesh only.
*CONTROL_FORMING_REMOVE_ADAPTIVE_CONSTRAINTS 
The  following  complete  input  file  converts  an  adaptive  mesh  file  blankadaptmsh.k 
(Figure  12-43  left)  with  the  PID  of  1  into  a  connected  mesh  (Figure  12-43  right).    The 
resulting mesh will be in the dynain file. 
*KEYWORD 
*INCLUDE 
blankadaptmsh.k 
*PARAMETER 
I blkpid           1 
$--------1---------2------- 
*CONTROL_TERMINATION 
0.0 
*CONTROL_FORMING_REMOVE_ADAPTIVE_CONSTRAINTS 
$   PID 
&blkpid 
*set_part_list 
1 
&blkpid 
*INTERFACE_SPRINGBACK_LSDYNA_NOTHICKNESS 
1 
*INTERFACE_SPRINGBACK_EXCLUDE 
INITIAL_STRAIN_SHELL 
INITIAL_STRESS_SHELL 
*PART 
$      PID       SID       MID 
   &blkpid         1         1                                        
*MAT_037 
... 
*SECTION_SHELL 
$    SECID    ELFORM      SHRF       NIP 
         1         2 0.000E+00         3 
1.0,1.0,1.0,1.0 
*END
Original mesh: adapt.msh
Modified, fully connected 
mesh: dynain
Figure 12-43.  Converting an adaptive mesh to a fully connected mesh. 
Revision information: 
This  feature  is  available  starting  from  LS-DYNA  Revision  108157,  in  both  SMP,  MPP, 
single and double precision.
*CONTROL_FORMING_SCRAP_FALL 
Purpose:  This keyword allows for direct and aerial trimming of a sheet metal part by 
trim steels in a trim die.  According to the trim steels and trim vectors defined, the sheet 
metal  part  will  be  trimmed  into  a  parent  piece  and  multiple  scrap  pieces.    The  parent 
piece  is  defined  as  a  fixed  rigid  body.    Trimmed  scraps  (deformable  shells)  are 
constrained along trim edges until they come into contact with the trim steel; the edge 
constraints  are  gradually  released  as  the  trim  steel’s  edge  contacts  the  scrap  piece, 
allowing for contact-based scrap fall simulation.  This keyword applies to shell elements 
only.  
Include  Card  1  columns  1-6  only  per  each  scarp  piece  for  the  constraint  release  method
.    For  the  scrap  trimming  method  include  one  set  of  Cards  1,  2  and  3  per 
trim steel.  The next “*” card terminates the input. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
VECTID 
NDSET 
LCID 
DEPTH 
DIST 
IDRGD 
IFSEED 
Type 
I 
I 
I 
I 
F 
F 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NOBEAD 
SEEDX 
SEEDY 
SEEDZ 
EFFSET 
GAP 
IPSET 
EXTEND 
Type 
I 
F 
F 
F 
F 
F 
I 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NEWID 
Type 
I 
Default 
none
VARIABLE   
PID 
VECTID 
NDSET 
DESCRIPTION
Part ID of a scrap piece.  This part ID becomes a dummy ID if
all trimmed scrap pieces are defined by NEWID.  See definition
for NEWID and Figure 12-46. 
Vector ID for a trim steel movement, as defined by *DEFINE_-
VECTOR.    If  left  undefined  (blank),  global  𝑧-direction  is 
assumed. 
A  node  set  consists  of  all  nodes  along  the  cutting  edge  of  the
trim  steel.    Note  that  prior  to  Revision  90339  the  nodes  in  the
set  must  be  defined  in  consecutive  order.    See  Remarks  (LS-
PrePost) below on how to define a node set along a path in LS-
PrePost.  This node set, together with VECTID, is projected to
the sheet metal to form a trim curve.  To trim a scrap out of a
parent  piece  involving  a  neighboring  trim  steel,  which  also
serves as a scrap cutter, the node set needs to be defined for the
scrap cutter portion only for the scrap, see Figure 12-46. 
LCID 
Load curve ID governing the trim steel kinematics, as defined
by *DEFINE_CURVE. 
DEPTH 
DIST 
IDRGD 
GT.0: velocity-controlled kinematics 
LT.0:  displacement-controlled kinematics 
An example input deck is provided below. 
A  small  penetrating  distance  between  the  cutting  edge  of  the
trim steel and the scrap piece, as shown in Figure 12-45.  Nodes 
along  the  scrap  edge  are  released  from  automatically  added
constraints  at  the  simulation  start  and  are  free  to  move  after
this distance is reached. 
A distance tolerance measured in the plane normal to the trim
steel  moving  direction,  between  nodes  along  the  cutting  edge
of the trim steel defined by NDSET and nodes along an edge of 
the  scrap,  as  shown  in  Figure  12-44.   This  tolerance  is  used  to 
determine if the constraints need to be added at the simulation
start to the nodes along the trim edge of the scrap piece. 
Part  ID  of  a  parent  piece,  which  is  the  remaining  sheet  metal
after  the  scrap  is  successfully  trimmed  out  of  a  large  sheet
metal.  Note the usual *PART needs to be defined somewhere
in  the  input  deck,  along  with  *MAT_20  and  totally  fixed
translational and rotational DOFs.  See Figure 12-46.
VARIABLE   
DESCRIPTION
IFSEED 
A flag to indicate the location of the scrap piece. 
EQ.0:  automatically  determined.    The  trim  steel  defined
will  be  responsible  to  trim  as  well  as  to  push  (have
contact with) the scrap piece. 
EQ.1:  automatically determined, however, the trim steel in
definition will only be used to trim out the scrap, not
to push (have contact with) the scrap piece. 
EQ.-1:  user  specified  by  defining  SEEDX,  SEEDY,  and
SEEDZ 
A  node  set  to  be  excluded  from  initially  imposed  constraints 
after trimming.  This node set typically consists of nodes in the
scrap  draw  bead  region  where  due  to  modeling  problems  the
beads on the scrap initially interfere with the beads on the rigid
tooling; it causes scrap to get stuck later in the simulation if left 
as is.  See Figure 12-47. 
NDBEAD 
SEEDX, SEEDY, 
SEEDZ 
𝑥,  𝑦,  𝑧  coordinates  of  the  seed  node  on  the  scrap  side;  define
only when IFSEED is set to “-1”.  See Figure 12-46. 
EFFSET 
GAP 
IPSET 
Scrap  edge  offset  amount  away  from  the  trim  steel  edge,
towards  the  scrap  seed  node  side.    This  is  useful  to  remove
initial  interference  between  the  trimmed  scrap  (because  of
poorly  modeled  trim  steel)  and  coarsely  modeled  lower  trim
post.  See Figure 12-46. 
Scrap  piece  offset  amount  from  the  part  set  defined  by  IPSET
(e.g.    top  surfaces  of  the  scrap  cutters),  in  the  direction  of  the
element normals of the IPSET.  This parameter makes it easier
to remove  initial  interference  between  the  scrap  and  other  die
components.  See Figure 12-48. 
A part set ID from which the scrap will be offset to remove the
initial  interference,  works  together  only  with  GAP.    The  part
set  ID  should  only  include  portions  of  tool  parts  that  are
directly underneath the scrap (top surface portion of the tools).
The  normals  of  the  IPSET  must  point  toward  the  scrap.    The
parts  that  should  belong  to  IPSET  are  typically  of  those
elements  on  the  top  surface  of  the  scrap  cutter,  see  Figure 
12-48.
The  Scrap  piece 
is 
modeled  as  a  deform-
able  shell  part;  parent 
piece does not need to 
be modeled.
Trim 
steel
Nodes  along  the  edge  of  the  trim 
steel  are  defined  in  a  sequentailly 
ordered node set.
Constraints 
automatically 
are 
generated  during  initilization  for 
the  nodes  in  blue  along  the  scrap 
trim edge, according to DIST.
GAP > 0.5 × (scrap thickness 
+ shell thickness of trim post)
Trim 
post
Trim line
DIST
Figure  12-44.    Modeling  details  of  the  constraint  release  method.    Drawing 
modified from the original sketches courtesy of the Ford Motor Company. 
  VARIABLE   
EXTEND 
NEWID 
Background: 
DESCRIPTION
An amount to extend a trim steel’s edge based on the NDSET
defined,  so  it  can  form  a  continuous  trim  line  together  with  a
neighboring  trim  steel,  whose  edge  may  also  be  extended,  to
trim out the scrap piece.  See Figure 12-46. 
New part ID of a scrap piece for the scrap area defined by the
seed location.  If this is not defined (left blank) or input as “0”,
the  scrap  piece  will  retain  original  PID  as  its  part  ID.    See
Figure 12-46.  This is useful in case where one original scrap is 
trimmed  into  multiple  smaller  pieces,  and  contacts  between
these smaller pieces need to be defined. 
Sheet  metal  trimming  and  the  resulting  scrap  fall  are  top  factors  in  affecting  the 
efficiency of stamping plants worldwide.  Difficult trimming conditions, such as those 
multiple  direct  trims,  a  mixture  of  direct  and  cam  trims,  and  multiple  cam  trims 
involving  bypass  condition,  can  cause  trimmed  scraps  to  get  stuck  around  and  never 
separate from the trim edge of the upper trim steels or lower trim post.  Inappropriate 
design of die structure and scrap chute can slow down or prevent scraps from tumbling 
out to the scrap collectors.  Smaller scrap pieces (especially aluminum)  can sometimes
shoot  straight  up,  and  get  stuck  and  gather  in  areas  of  the  die  structure.    All  these 
problems  result  in  shutdowns  of  stamping  presses,  reducing  stroke-per-minute  (SPM) 
and causing hundreds of thousands of dollars in lost productivity. 
With this keyword, engineers can consider the trimming details, manage the scrap trim 
and  the  drop  energy,  study  different  trimming  sequences,  explore  better  die  structure 
and  scrap  chutes  design  and  layout  before  a  trim  die  is  even  built.    This  feature  is 
developed in conjunction with the Ford Motor Company. 
The constraint release method: 
Prior  to  Revision  91471  ,  simulating  the  scrap  trim  and  fall  uses  the 
“constraint release” method, where only the scrap piece is modeled and defined.   
As shown in Figure 12-44, the scrap piece is modeled as a deformable body and the trim 
steel  and  trim  post  as rigid  shell  elements,  while  the  parent  piece  does  not  need  to  be 
modeled at all.  Between the trim edge of the scrap piece and the post there should be a 
gap (indicated by GAP in the figure).  The gap ensures that the contact interface (to be 
explained later) correctly accounts for the shell thickness along the edge.  A gap that is 
too  small  may  cause  initial  penetration  between  the  scrap  and  the  post  which  may 
manifest as unphysical adhesion between the scrap and the post.
The Scrap piece
Trim 
steel
Cutting Tolerance. When a 
portion  of  the  trim  steel 
comes  within  DEPTH  of 
a  constrained  node,  the 
constraint  is  released.  In 
the  above  schematic  the  tolerance  is 
indicated by the highlighted region.
Constraint  release  (final).    Last  contacted  node 
along  the  trim  line  gets  released  last  from  the 
constraints.
Trim line
Trim 
post
Constraint  release  (start).    First  node  in  contact  is  the  first 
released from constraints.  The motion of the trim steel is 
carried onto the scrap piece by the contact interface.
Figure  12-45.    Contact-based  separation  and  contact-driven  kinematics  and 
dynamics  in  the  constraint  release  method.    Drawing  modified  from  the  original 
sketches courtesy of the Ford Motor Company. 
The  edge  of  the  scrap  piece  should  initially  be  flush  with  that  of  the  trim  post 
(perpendicular  to  the  trim  direction),  just  as  exactly  what  happens  in  the  production 
environment.    If  the  scrap  is  unrealistically  positioned  above  the  trim  post  edge,  the 
scrap  may  be  permanently  caught  between  the  trim  steel  and  the  post  under  a 
combination of uncertain trimming forces as the trim steel moves down. 
During initialization, constraints are added automatically on the nodes along the scrap 
trim  edge  corresponding  to  the  node  set  (NDSET)  along  the  trim  steel,  based  on  the 
supplied  tolerance  variable  DIST  and  trim  vector  VECTID.    Although  the  direction  of 
the path is not important, prior to Revision 90339, the NDSET must be arranged so that 
the  nodes  are  in  a  sequential  order  (LS-PrePost  4.0  creating  node  set  by  path).    As  the 
edge of the trim steel comes within DEPTH distance of the trim line, the constraints are 
removed.    The  contact  interfaces  serve  to  project  the  motion  of  the  trim  steel  onto  the 
scrap piece, see Figure 12-45. 
The scrap trimming method: 
The original simplified method has the following drawbacks:
1.  No scrap trimming – the scrap piece cannot be trimmed directly from a parent 
piece; an exact scrap piece after trimming must be modeled. 
2.  Poorly (or coarsely) modeled draw beads in the scrap piece do not fit properly 
in  badly  modeled  draw  beads  on  the  tooling,  resulting  in  initial  interferences 
between the two and therefore affecting the simulation results. 
3.  For  poorly  (or  coarsely)  modeled  scrap  edges  and  trim  posts,  users  have  to 
manually  modify  the scrap  trim  edges to  clear  the  initial  interference  with  the 
trim posts. 
4.  Users  must  clear  all  other  initial  interferences  (e.g.    between  scrap  and  scrap 
cutter) manually. 
Based  on  users’  feedback,  a  new  method  “scrap  trimming”  (after  Revision  91471)  has 
been  developed  to  address  the  above  issues  and  to,  furthermore,  reduce  the  effort 
involved  in  preparing  the  model.    The  new  method  (Figure  12-46)  involves  trimming 
scrap  from  an  initially  large  piece  of  sheet  metal,  leaving  the  parent  piece  as  a  fixed 
rigid body.  The trim lines are obtained from the trim steel edge node set NDSET and 
the trim vector VECTID. 
Parameters related to the constraint release method: 
1.  The value of DEPTH is typically set to one-half of the scrap thickness. 
2.  The  initial  gap  separating  the  scrap  from  the  post  must  be  greater  than  the 
average of the scrap and post thickness values, see Figure 12-44. 
3.  The  input  parameter  DIST  should  be  set  larger  than  the  maximum  distance 
between nodes along the trim steel edge and scrap edge in the view along the 
trim direction, see Figure 12-44. 
Parameters related to the scrap trimming method: 
4.  Similar  to  DEPTH,  EFFSET  should  be  typically  set  to  one-half  of  the  scrap 
thickness,  although  it  may  be  larger  for  some  poorly  modeled  trim  steels  and 
trim posts.  
Contact: 
Only  *CONTACT_FORMING  contact  interfaces  are  allowed  for  contact  between  the 
scrap piece and the trim steel.  In particular, *CONTACT_FORMING_SURFACE_TO_-
SURFACE  is  recommended.    A  negative  contact  offset  must  be  used;  this  is  done
typically  by  setting  the  variable  MST  in  *CONTACT_FORMING_SURFACE_TO_SUR-
FACE to the negative thickness value of the scrap piece. 
For  contact  between  the  scrap  piece  and  the  shell  elements  in  all  the  other  die 
structures, *CONTACT_AUTOMATIC_GENERAL should be used for the edge-to-edge 
contact  frequently  encountered  during  the  fall  of  the  scrap  piece.    All  friction 
coefficients  should  be  small.    The  explicit  time  integrator  is  recommended  for  the 
modeling of scrap trim and fall.  Mass scaling is not recommended. 
LS-PrePost: 
The node set (NDSET) defined along the trim steel edge can be created with LS-PrePost 
4.0,  via  Model/CreEnt/Cre,  Set  Data,  *SET_NODE,  ByPath,  then  select  nodes  along  the 
trim edge continuously until finish and then hit Apply. 
Keyword examples – the constraint release method: 
A  partial  example  of  using  the  keyword  below  includes  a  node  set  ID  9991  along  the 
trim steel (PID 2) edge used to release the constraints between the scrap piece with PID 
1, and the parent piece.  The LCID for the trim steel kinematics  is (+)33 (load  curve is 
controlled  by  velocity)  moving  in  –Z  direction.    The  trimming  velocity  is  defined  as 
1000 mm/s and the retracting velocity is 4000 mm/s.  The variables DEPTH and DIST 
are  set  to  0.01  and  2.5,  respectively.    The  contact  interface  between  the  trim  steel  and 
scrap  piece  is  defined  using  *CONTACT_FORMING_SURFACE_TO_SURFACE  and 
contact between the scrap and all other die structures are defined using *CONTACT_-
AUTOMATIC_GENERAL. 
*KEYWORD   
*CONTROL_TERMINATION 
&endtime 
*CONTROL_FORMING_SCRAP_FALL 
$      PID    VECTID     NDSET      LCID     DEPTH      DIST 
         1                9991        33      0.75      2.0  
*SET_NODE_LIST 
      9991 
     24592     24591     24590     24589     24593     24594     24595     24596 
*BOUNDARY_PRESCRIBED_MOTION_rigid 
$pid,dof,vad,lcid,sf,vid,dt,bt 
2,3,0,33,-1.0 
*DEFINE_CURVE 
33 
0.0,0.0 
0.216,1000.0 
0.31,-4000.0 
0.32,0.0 
0.5,0.0 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*CONTACT_forming_surface_to_surface_ID 
         1 
         1         2         3         3         0         0         0         0 
      0.02       0.0       0.0       0.0      20.0         0       0.01.0000E+20 
$#     sfs       sfm       sst       mst      sfst      sfmt       fsf       vsf
0.0       0.0       0.0      &mst       1.0       1.0       1.0       1.0 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*CONTACT_AUTOMATIC_GENERAL_ID 
         2 
*END 
For the negative option of LCID, displacement will be used as input to control the tool 
kinematics.  A partial example is provided below, where LCID is defined as a negative 
integer of a load curve, controlling the trim steel kinematics.  The trim steel is moving 
down  for  27.6075  mm  in  0.2  sec  to  trim,  and  moving  up  for  the  same  distance  to  its 
original  position  in  0.3  sec  to  retract.    Although  this  option  is  easier  to  use,  the 
corresponding  velocity  from  the  input  time  and  displacement  must  be  realistic  for  a 
realistic simulation. 
*CONTROL_FORMING_SCRAP_FALL 
$ LCID<0: trimming steel kinematics is controlled by displacement. 
$      PID    VECTID     NDSET      LCID     DEPTH      DIST 
         1        44         1    -33332      0.70      2.00 
*DEFINE_VECTOR 
44,587.5,422.093,733.083,471.104,380.456,681.412 
*BOUNDARY_PRESCRIBED_MOTION_rigid_LOCAL 
$pid,dof,vad,lcid,sf,vid,dt,bt 
11,3,2,33332,1.0,44 
*DEFINE_CURVE 
33332 
0.0,0.0 
0.2,-27.6075 
0.5,0.0 
A keyword example – the scrap trimming method: 
The keyword example below shows three scrap pieces, with original PID &SPID1, new 
PIDs 1001 and 1002, being trimmed out of a larger scrap &SPID1;  the remaining parent 
piece is defined as a fixed rigid body with PID 110.  A different seed location is defined 
separately for each scrap.  The scraps &SPID1, 1001 and 1002 are each offset by 0.60mm 
in the area of the seed location defined, in the direction normal to the elements defined 
by IPSET 887, 888, and 889, respectively.  The trim edge offset is 0.90mm for all scraps.  
The draw bead node sets to be released are, 987, 988, 989 for each scrap as defined by 
the corresponding seed locations. 
*CONTROL_FORMING_SCRAP_FALL 
$      PID    VECTID     NDSET     VLCID     DEPTH      DIST     IDRGD    IFSEED 
    &spid1    &cord1    &nset1      1800   &depth1      2.00       110        -1 
$   NDBEAD     seedx     seedy     seedz    effset       GAP     IPSET    EXTEND 
       987  -528.046    373.40   710.000      0.90      0.60       887       8.0 
         0 
    &spid1    &cord2    &nset2      1801   &depth1      2.00       110        -1 
       987  -528.046    373.40   710.000      0.90      0.60       887       8.0 
         0 
    &spid1    &cord3    &nset3      1802   &depth1      2.00       110        -1 
       987  -528.046    373.40   710.000      0.90      0.60       887       8.0 
         0 
$ 
    &spid1    &cord3   &nset33      1802   &depth1      2.00       110        -1 
       988  -252.452   383.322   799.974      0.90      0.60       888       8.0
1001 
    &spid1    &cord4    &nset4      1803   &depth1      2.00       110        -1 
       988  -252.452   383.322   799.974      0.90      0.60       888       8.0 
      1001 
    &spid1    &cord5    &nset5      1804   &depth1      2.00       110        -1 
       988  -252.452   383.322   799.974      0.90      0.60       888       8.0 
      1001 
$ 
    &spid1    &cord5   &nset55      1804   &depth1      2.00       110        -1 
       989    74.452   404.522   857.974      0.90      0.60       889       8.0 
      1002 
    &spid1    &cord6    &nset6      1805   &depth1      2.00       110        -1 
       989    74.452   404.522   857.974      0.90      0.60       889       8.0 
      1002 
    &spid1    &cord7    &nset7      1806   &depth1      2.00       110        -1 
       989    74.452   404.522   857.974      0.90      0.60       889       8.0 
      1002 
Revision/Other information: 
A graphical user interface capable of setting up a complete input deck for the original 
simplified  method  is  now  available  in  LS-PrePost  4.0  under  APPLICATION/Scrap  Trim 
reference  paper 
(http://ftp.lstc.com/anonymous/outgoing/lsprepost/4.1/). 
regarding  the  development  and  application  of  this  keyword  for  the  constraint  release 
method  can  be  found  in  the  proceedings  of  the  12th  International  LS-DYNA  User's 
Conference.  The following provides a list of revision history for the keyword: 
  A 
1.  The constraint release method is available between LS-DYNA Revision 63618 and 
91471. 
2.  The scrap trimming method is available starting in Revision 91471. 
3.  The parameter NEWID is available starting in Revision 92578. 
4.  The  restriction  of  NDSET  must  be  defined  in  a  consecutive  order  is  lifted 
starting in Revision 90339.
IDRGD
Trim steel 1
Trim steel 2
NEWID2
NEWID1 or PID 
NEWID3
Scrap cutter
Scrap seed node
EXTEND
EXTEND
IDRGD
NSET1
Trim steel 1
NEWID2
EFFSET
NSET2
SEEDX, Y, Z
Trim steel 2
Figure  12-46.    Trimming  of  multiple  scraps  and  parameter  definitions  in  the
scrap trimming method.  Model courtesy of the Ford Motor Company.
NDBEAD
NDBEAD
Figure  12-47.    Definition  of  NDBEAD  in  the  scrap  trimming  method.    Model
courtesy of the Ford Motor Company.
Scrap piece
Scrap cutter 
top surface
Before trim
Scrap cutter side view
Element normals
Scrap piece: Normals should face the IPSET
GAP
IPSET:  To  get 
the  proper  offset,  elements 
immediately  below  the  scrap  piece  should  be 
separated  into  a  different  PID  (and  included  in 
the  IPSET)  from  the  vertical  walls  of  the  scrap 
cutter.  In addition, IPSET should have consistent 
normals pointing toward the scrap piece. 
After trim
Figure  12-48.    Element  normal  of  the  IPSET  in  the  scrap  trimming  method.
Model courtesy of the Ford Motor Company.
*CONTROL_FORMING_SHELL_TO_TSHELL 
Purpose:  This keyword is created to allow users to easily change the element type from 
thin  shell  elements  (*SECTION_SHELL)  to  thick  shell  elements  (*SECTION_TSHELL), 
and  to  generate  segments  on  both  top  and  bottom  side  of  the  thick  shells.    Note  that 
mesh adaptivity is also supported. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
THICK 
MIDSF 
IDSEGB 
IDSEGT 
Type 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
PID 
Part ID of the thin shell elements. 
THICK 
Thickness of the thick shell elements (Tshell). 
MIDSF 
Tshell mid-plane position definition : 
IDSEGB 
MIDSF.EQ.0:  Mid-plane is at thin shell surface. 
MIDSF.EQ.1:  Mid-plane  is  at  one  half  of  THICK  above  thin 
shell surface. 
MIDSF.EQ.-1:  Mid-plane  is  at  one  half  of  THICK  below  thin 
shell surface. 
Set ID of the segments to be generated on the bottom layer of the
Tshells,  which  can  be  used  for  segment-based  contact.    The 
bottom side of Tshells is the opposite side of the positive normal
side of the thin shells, see Figure 12-49. 
Note the default normal of the generated segments are consistent
with  the  thin  shells’  normal.    To  reverse  this  default  normal,  set
the IDSEGB to a negative number. 
Under  the  FORMING  type  of  contact,  if  the  generated  segments
are used as a slave member in contact with a master member of a 
rigid  body,  the  rigid  body’s  normals  must  be  consistent  and
facing the slave segments.  Note that the slave segments normals
are not required to point at the rigid bodies, although they should
be made consistent.
IDSEGT 
*CONTROL_FORMING_SHELL_TO_TSHELL 
DESCRIPTION
Set  ID  of  the  segments  to  be  generated  on  the  top  layer  of  the
Tshells,  which  can  be  used  for  segment-based  contact.    The  top 
side of a Tshells is the same side of the positive normal side of the
thin shells, see Figure 12-49. 
Note  the  normal  of  the  generated  segments  are  consistent  with
the  thin  shells’  normal.    To  reverse  this  default  normal,  set  the
IDSEGT to a negative number. 
Remarks: 
This keyword will convert thin shell elements to thick shell elements.  The position of 
the  thick  shells’  mid-plane  in  reference  to  the  thin  shell’s  surface  is  dependent  on 
MIDSF (Figure 12-49).  Node IDs of the thick shell elements will be the same as those for 
the  thin  shells.    Element  IDs  of  the  thick  shell  elements  will  start  at  2  (so  renumber 
element IDs of other PID accordingly).  Only one layer of thick shells will be created. 
New nodes generated adaptively from their parent nodes with *BOUNDARY_SPC are 
automatically constrained accordingly. 
This feature is developed as requested by JSOL Corporation. 
Examples: 
1)A  standalone  part  of  thin  shell  elements  can  be  changed  to  thick  shell  elements 
with  a  simplified  small  input  deck.    The  following  will  convert  shell  elements 
with  PID  100  of  thickness  1.5mm  to  thick  shell  elements  of  PID  100  with  thick-
ness of 2.0mm, with thick shell meshes stored in a file “dynain.geo”.  Note that 
MIDSF, IDSEGB and IDSEGT cannot be used in this case. 
*KEYWORD 
*CONTROL_TERMINATION 
0.0 
*INCLUDE 
shellupr.k 
*SET_PART_LIST 
1, 
100 
*PART 
Sheet blank 
100,100,100 
*SECTION_SHELL 
$      SID    ELFORM      SHRF       NIP     PROPT 
       100         2     0.833         3       1.0 
$       T1        T2        T3        T4      NLOC 
1.5,1.5,1.5,1.5 
*MAT_037 
$#     MID        RO         E        PR      SIGY      ETAN         R     HLCID 
100        7.8500E-9 2.1000E+5  0.333000                          1.00     90905
*DEFINE_CURVE 
     90905  
     0.000000000E+00     0.380000000E+03 
     0.300000003E-02     0.392489226E+03 
     0.600000005E-02     0.403294737E+03 
     0.899999961E-02     0.412847886E+03 
     0.120000001E-01     0.421429900E+03 
     0.150000006E-01     0.429234916E+03 
     0.179999992E-01     0.436402911E+03 
     0.209999997E-01     0.443038343E+03 
*INTERFACE_SPRINGBACK_LSDYNA 
1 
OPTCARD,,,1 
*CONTROL_FORMING_SHELL_TO_TSHELL 
$      PID     THICK 
       100       2.0 
*END 
that 
2)The  conversion  can  also  be  done  in  an  input  deck  set  up  for  a  complete  metal 
forming  simulation  with  thin  shell  elements  as  a  sheet  blank.    The  conversion 
happens  in  the  beginning  of  the  simulation,  as  shown  in  an  example  below.  
Only  the  keywords  needed  change  are  listed,  commented  out  with  $  signs  and 
replaced with appropriate cards for thick shells.  The thin shell sheet blank with 
PID  1  is  to  be  converted  to  a  thick  shell  sheet  blank  with  thickness  of  1.6mm, 
noting 
instead  of 
*SECTION_SHELL  for  the  sheet  blank.    Corresponding  material  type  for  the 
sheet  blank  (*MAT_037)  also  needs  to  be  changed  to  a  type  that  supports  solid 
element  simulation  (*MAT_024).    The  mid-plane  of  the  thick  shells  will  be  one 
half of 1.6 mm below the thin shells’ surface, with segment IDs 10 (IDSEGB) and 
11 (IDSEGT) created on the bottom and top side of the thick shells, respectively, 
as shown in Figure 12-49.  IDSEGB 10 with SSTYP 0 is defined to contact with the 
lower punch (part set ID 2) with MSTYP 2, and IDSEGT 11 with SSTYP 0 is used 
for contact with the upper die cavity with part set ID of 3, of MSTYP 2.  
should  be  defined 
*SECTION_TSHELL 
the 
*KEYWORD 
... 
*PART 
Sheet blank 
1,1,1 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
$                    Blank property 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
$*SECTION_SHELL 
$      SID    elform      SHRF       nip     PROPT   QR/IRID     ICOMP     SETYP 
$        1         2     0.833         3       1.0 
$       T1        T2        T3        T4      NLOC 
$&b1thick,&b1thick,&b1thick,&b1thick 
*SECTION_TSHELL 
$      SID    elform      SHRF       nip     PROPT   QR/IRID     ICOMP     SETYP 
         1         1     0.833      &nip       1.0 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
$*MAT_037 
$      MID        RO         E        PR      SIGY      ETAN         R     HLCID 
$        1  7.85E-09  2.07E+05      0.28                                      92 
*MAT_024 
$      MID        RO         E        PR      SIGY      ETAN      FAIL      TDEL 
         1  7.85E-09  2.07E+05      0.28     382.8       0.0       0.0       0.0 
$        C         P      LCSS      LCSR        VP
0.0       0.0        92         0       0.0 
$     EPS1      EPS2      EPS3      EPS4      EPS5      EPS6      EPS7      EPS8 
$      ES1       ES2       ES3       ES4       ES5       ES6       ES7       ES8 
*DEFINE_CURVE 
92,,,0.5 
    0.0000000000E+00    3.8276000000E+02 
    4.0000000000E-03    3.9616000000E+02 
8.0000000000E-03    4.0695000000E+02 
           ⋮                    ⋮ 
*INTERFACE_SPRINGBACK_LSDYNA 
1 
OPTCARD,,,1 
*CONTROL_FORMING_SHELL_TO_TSHELL 
$      PID     THICK     MIDSF    IDSEGB    IDSEGT 
       100       1.6        -1        10        11 
*CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE 
$     SSID      MSID     SSTYP     MSTYP 
        11         2         0         2 
         ⋮          ⋮         ⋮ 
*CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE 
$     SSID      MSID     SSTYP     MSTYP 
        10         3         0         2 
         ⋮          ⋮         ⋮ 
... 
*END 
Revision information: 
This  feature  is  available  in  LS-DYNA  starting  in  Revision  104903.    The  following 
revisions indicate the Revision history of additional features: 
1)  Revision 106116: negative option of IDSEGB and IDSEGT. 
2)  Revision 106162: MIDSF, IDSETGB and IDSEGT becomes available. 
3)  Revision:  106217:  automatically  add  *BOUNDARY_SPC  for  newly  generated 
nodes  whose parent nodes are assigned with *BOUNDARY_SPC.
Thin shell 
normals
Original sheet blank 
with shell elements
Thin shell 
surface
Created thick shells for 
MIDSF=0
Thick shell 
mid-plane
THICK
THICK
THICK
Created thick shells for 
MIDSF=1
Thick shell 
mid-plane
Created thick shells for 
MIDSF=-1
Thick shell 
mid-plane
NUMISHEET'05 Cross member
Top segment ID 11
(IDSEGT)
Bottom segment ID 10
(IDSEGB)
  Figure 12-49.  Converting thin shells to thick shells in sheet metal forming
*CONTROL_FORMING_STONING 
Purpose:    This  feature  is  developed  to  detect  surface  lows  or  surface  defects  formed 
during  metal  stamping.    This  calculation  is  typically  performed  after  a  springback 
simulation.    A  curvature-based  method  is  implemented  with  the  feature.    Users  have 
the option to check an entire part or just a few local areas, defined by node set or shell 
element set.  In each area, direction of the stoning action can be specified by two nodes 
  or  simply  allow  the  program  to  automatically  determine  the 
stoning direction. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ISTONE 
LENGTH  WIDTH 
STEP 
DIRECT  REVERSE  METHOD 
Type 
I 
F 
F 
F 
F 
Default 
none 
0.0 
0.0 
0.0 
0.0 
  Card 2 
1 
2 
3 
4 
Variable 
NODE1 
NODE2 
SID 
ITYPE 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
5 
V1 
F 
0.0 
0.0 
0.0 
I 
0 
6 
V2 
F 
I 
0 
7 
V3 
F 
8 
  VARIABLE   
DESCRIPTION
ISTONE 
Stoning calculation option. 
EQ.1: calculate panel surface quality using stoning method. 
LENGTH 
Length of the stone. 
WIDTH 
Width of the stone. 
STEP 
Stepping size of the moving stone. 
DIRECT 
Number of automatically determined stoning direction(s).
VARIABLE   
DESCRIPTION
REVERSE 
Surface normal reversing option: 
EQ.0: do not reverse surface normals. 
EQ.1: reverse surface normals. 
METHOD 
Stoning method. 
EQ.0: curvature-based method. 
NODE1 
Tail node defining stoning moving direction. 
NODE2 
Head node defining stoning moving direction. 
SID 
Node or shell set ID. 
ITYPE 
Set type designation: 
EQ.1: node set 
EQ.2: element set 
V1, V2, V3 
Vector components defining stoning direction (optional). 
About stoning: 
Stoning is a quality checking process on class-A exterior stamping panels.  Typically the 
long and wider surfaces of an oil stone of a brick shape are used to slide and scratch in a 
given direction against a localized area of concern on a stamped panel.  Surface “lows” 
are  shown  where  scratch  marks  are  not  visible  and  “highs”  are  shown  in  a  form  of 
scratch  marks.    This  keyword  is  capable  of  predicting  both  the  surface  “lows”  and 
“highs”.    Since  stoning  process  is  carried  out  after  the  stamping  (either  drawn  or 
trimmed) panels are removed from the stamping dies, a springback simulation needs to 
be performed prior to conducting a stoning analysis. 
Modeling guidelines: 
As  a  reference,  typical  stone  length  and  width  can  be  set  at  150.0  and  30.0  mm, 
respectively.  The step size of the moving stone is typically set about the same order of 
magnitude  of  the  element  length.    The  smallest  element  length  can  be  selected  as  the 
step size. 
The variable DIRECT allows for the automatic definition of the stoning directions.  Any 
number  can  be  selected  but  typically  2  is  used.    Although  CPU  time  required  for  the 
stoning calculation is trivial, a larger DIRECT consumes more CPU time.
Stoning is performed on the outward normal side of the mesh.  Element normals must 
be  consistent  and  oriented  accordingly.    Element  normal  can  be  automatically  made 
consistent  in  LS-PrePost4.0  under  EleTol/Normal  menu.    Alternatively,  the  variable 
REVERSE provides in the solver an easy way to reverse a part with consistent element 
normals before the computation. 
The variables NODE1 and NODE2 are used to define a specific stoning direction.  The 
stone is moved in the direction defined by NODE1 to NODE2.  Alternatively, one can 
leave  NODE1  and  NODE2  blank  and  define  the  number  of  automatically  determined 
stoning directions by  using the variable DIRECT.  Furthermore, stoning direction  can 
also be defined using a vector by defining the variables V1, V2, and V3. 
The blank model intended for analysis can be included using keyword *INCLUDE.  If 
nothing is defined for SID and ITYPE then the entire blank model included will be used 
for stoning analysis. 
A large area mesh can be included in the input file.  An ELSET must also be included, 
which defines a local area that requires stoning computation.  Alternatively, an ELSET 
can define several local areas to be used for the computation.  Furthermore, an ELSET 
should  not  include  meshes  that  have  reversed  curvatures.    An  ELSET  can  be  easily 
generated using LS-PrePost4.0, under Model/CreEnt/Cre/Set_Data/*SET_SHELL. 
Since  stoning  requires  high  level  of  accuracy  in  springback  prediction,  it  is 
recommended  that  the  SMOOTH  option  in  keyword  *CONTACT_FORMING_ONE_-
WAY_SURFACE_TO_SURFACE to be used during the draw forming simulation.  Not 
all  areas  require  SMOOTH  contact,  only  areas  of  interest  may  apply.    In  addition, 
meshes in the areas of concern need to be very fine, with average element size of 1 to 2 
mm.  Mesh adaptivity is not recommended in the SMOOTH/stoning areas.  Also, mass 
scaling with DT2MS needs to be sufficiently small to reduce the dynamic effect during 
forming.  For binder closing of large exterior panels, implicit static method using *CON-
TROL_IMPLICIT_FORMING  type  2  is  recommended,  to  further  reduce  potential 
buckles caused by the inertia effect. 
Stoning results/output: 
It  is  recommended  that  double  precision  version  of  LS-DYNA  be  used  for  this 
application.    The  output  of  the  stoning  simulation  results  is  in  a  file  named 
“filename.output”,  where  “filename”  is  the  name  of  the  LS-DYNA  stoning  input  file 
containing this keyword, without the file extension.  The stoning results can be viewed 
using LS-PrePost4.0, under MFPost/FCOMP/Shell_Thickness.
Application example: 
An example of a stoning analysis on a Ford Econoline door outer panel is provided for 
reference.    The  original  part  model  comes  from  National  Crash  Analysis  Center  at  The 
George  Washington  University.    The  original  part  was  modified  heavily  in LS-PrePost4.0 
to fit the needs of the demonstration purpose.  Binder and addendum were created and 
sheet  blank  size  was  assumed.    The  blank  is  assigned  0.65mm  thickness  and  a  BH210  
properties  with  *MAT_037.    Shell  thickness  contour  plots  for  the  drawn  and  trimmed 
panels are shown in Figures 12-50 and 12-51, respectively.  Springback amount in Z is 
plotted  in  Figure  12-52.    The  complete  input  deck  used  for  the  stoning  simulation  is 
provided  below  for  reference;  where,  a  local  area  mesh  of  the  door  handle  after 
springback simulation “Doorhandle.k” and an element set “elset1.k” are included in the 
deck.    Locations  of  the  ELSETs  are  defined  for  the  upper  right  (Figure  12-53  left)  and 
lower  right  corners  (Figure  12-54  left)  of  the  door  handle,  where  “mouse  ear”  are 
expected. 
*KEYWORD 
*TITLE 
Stoning Analysis 
*INCLUDE 
Doorhandle.k 
*INCLUDE 
elset1.k 
*CONTROL_FORMING_STONING 
$   ISTONE    LENGTH     WIDTH      STEP    DIRECT   REVERSE    METHOD 
         1     150.0       4.0       1.0         9         0         0 
$    NODE1     NODE2       SID     ITYPE 
                             1         2 
*END 
Stoning results are shown in Figures 12-53 (right) and 12-54 (right) for the upper right 
and lower right corners, respectively.  “Mouse ears” are predicted where anticipated. 
Revision information: 
The stoning feature is available in LS-DYNA Revision 54398 and later releases.  Vector 
component option is available in Revision 60829 and later releases.
Thickness (mm)
0.6818
0.6649
0.6480
0.6310
0.6141
0.5972
0.5803
0.5634
0.5464
0.5295
0.5126
Figure 12-50.  Thickness contour of the panel after draw simulation. 
Thickness (mm)
0.6818
0.6649
0.6480
0.6310
0.6141
0.5972
0.5803
0.5634
0.5464
0.5295
0.5126
Figure 12-51.  Thickness contour of the panel after trimming.
Springback (mm)
0.6818
0.6649
0.6480
0.6310
0.6141
0.5972
0.5803
0.5634
0.5464
0.5295
0.5126
Figure 12-52.  Springback amount (mm). 
A region where an "elset" 
was selected for stoning
Stoning results: "mouse 
ear" potential in the corner
Out-of-plane 
displacement 
(mm)
0.2336
0.2103
0.1869
0.1636
0.1402
0.1166
0.0935
0.0070
0.0467
0.0234
0.0000
Figure 12-53.  Stoning simulation for the upper right door corner.
Out-of-plane 
displacement 
(mm)
0.3580
0.3222
0.2864
0.2506
0.2148
0.1790
0.1432
0.1074
0.0716
0.0358
0.0000
A region where another "elset" 
was defined for stoning 
Stoning results: "mouse ear" 
potential in the corner 
Figure 12-54.  Stoning simulation for the lower right door corner.
*CONTROL_FORMING_TEMPLATE 
Purpose:  This keyword is used to simplify the required input for sheet metal stamping 
simulations.    With  this  keyword,  five  templates  are  given: three-piece  air  draw,  three-
piece toggle draw, four-piece stretch draw, trimming, and springback. 
NOTE:  This  option  has  been  deprecated  in  favor  of  *CON-
TROL_FORMING_AUTOPOSITION_PARAME-
TER. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IDTEMP 
BLKID 
DIEID 
PNCH 
BNDU 
BNDL 
TYPE 
PREBD 
Type 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
I 
0 
F 
0.0 
Remarks 
1 
  Card 2 
1 
2 
2 
3 
4 
5 
Variable 
LCSS 
AL/FE 
R00 
R45 
R90 
Type 
I 
C 
F 
F 
F 
6 
E 
F 
7 
8 
DENSITY 
PR 
F 
F 
Default 
none 
Fe 
1.0 
R00 
R00 
none 
none 
none 
  Card 3 
Variable 
Type 
1 
K 
F 
2 
N 
F 
3 
4 
5 
6 
MTYP 
UNIT 
THICK 
GAP 
I 
F 
F 
8 
7 
FS 
F 
Default 
none 
none 
37 
none 
1.1t 
0.1 
I
Card 4 
1 
2 
Variable 
PATERN 
VMAX 
Type 
Default 
I 
1 
F 
1000 
  Card 5 
1 
2 
3 
VX 
F 
0 
3 
4 
VY 
F 
0 
4 
5 
VZ 
F 
6 
7 
8 
VID 
AMAX 
I 
F 
-1 
none 
1.0e+6 
5 
6 
7 
8 
Variable 
LVLADA 
SIZEADA  TIMSADA
D3PLT 
Type 
Default 
I 
1 
F 
I 
I 
none 
20 
10 
  VARIABLE   
DESCRIPTION
IDTEMP 
Type of forming process: 
EQ.1: 3-piece air-draw (Figure 12-55) 
EQ.2: 3-piece Toggle-draw (Figure 12-56) 
EQ.3: 4-piece stretch draw (Figure 12-57) 
EQ.4: Springback 
EQ.5: Trimming 
BLKID 
Part or part set ID  that defines the blank. 
DIEID 
Part  or  part  set  ID  that  defines  the  die.    See  Figures  12-55,  12-56
and 12-57 for more information 
PNCHID 
Part or part set ID that defines the punch. 
BNDUID 
Part or part set ID that defines the upper binder. 
BNDLID 
Part or part set ID that defines the lower binder.
Upper die (cavity)
Blank
Punch
(post)
Lower
binder
Binder gap
(a) Positioning
(b) Binder closing
(c) Forming
Figure 12-55.  IDTEMP = 1: forming in 3-piece air draw. 
Upper
binder
Punch
(Post)
Blank
Lower die
(cavity)
Binder gap
(a) Positioning
(b) Binder closing
(c) Forming
Figure 12-56.  IDTEMP = 2: forming in 3-piece toggle draw. 
  VARIABLE   
TYPE 
DESCRIPTION
Flag  for  part  or  part  set  ID  used  in  the  definition  of  BLKID,
DIEID, PNCHID, BNDUID, and BNDLID: 
EQ.0: Part ID 
EQ.1: Part set ID 
PREBD 
LCSS 
“Pull-over”  distance,  for  4  piece  stretch  draw  only.    This  is  the
travel distance of both upper and lower binder together after they
are  fully  closed.    Typically  this  distance  is  below  50mm.    See
Figure 12-57 for more information. 
If  the  material  (*MAT_XXX)  for  the  blank  is  not  defined,  this 
curve ID will define the stress-strain relationship; otherwise, this 
curve is ignored.
Upper
punch
Blank
Lower die
(cavity)
Upper
binder
Lower
binder
Binder
gap
PREBD
(a) Positioning
(b) Binder closing
(c) Pull-over
(d) Upper closing
(e) Draw home
Figure 12-57.  IDTEMP = 3: forming in 4-piece stretch draw. 
  VARIABLE   
AL/FE 
DESCRIPTION
This  parameter  is  used  to  define  the  Young’s  Modulus  and
density of the blank.  If this parameter is defined, E and DENSITY
will be defined in the units given by Table 12-58. 
EQ.A:  the blank is aluminum  
EQ.F:  the blank is steel (default) 
R00, R45, 
R90 
Material anisotropic parameters.  For transversely anisotropy the
R value is set to the average value of R00, R45, and R90.  
E 
Young’s Modulus.  If AL/FE is user defined, E is unnecessary 
DENSITY 
Material  density  of  blank.    If  AL/FE  is  user  defined,  this
parameter is unnecessary 
PR 
K 
Poisson’s ratio. 
Strength coefficient for exponential hardening (𝜎̅̅̅̅̅ = 𝑘𝜀̅ 𝑛).  If LCSS 
is  defined,  or  if  a  blank  material  is  user  defined  by  *MAT_XXX,
this parameter is ignored.
VARIABLE   
DESCRIPTION
N 
MTYP 
UNIT 
THICK 
GAP 
Exponent  for  exponential  hardening  (𝜎̅̅̅̅̅ = 𝑘𝜀̅ 𝑛).    If  LCSS  is 
defined,  or  if  a  blank  material  user  defined,  this  parameter  is
ignored. 
Only material models *MAT_036 and *MAT_037 are supported. 
Define  a  number  between  1  and  10  (Table  12-58)  to  indicate  the 
UNIT used in this simulation.  This unit is used to obtain proper
punch velocity, acceleration, time step, and material properties. 
Blank  thickness.    If  the  blank  thickness  is  already  defined  with
*SECTION_SHELL, this parameter is ignored. 
The gap between rigid tools at their home position.  If *BOUND-
ARY_PRESCRIBED_RIGID_BODY is user defined, this parameter 
is ignored.  The default is 1.1 x blank thickness. 
FS 
Friction coefficient (default = 0.10).  If the contact (*CONTACT) is 
user defined, this parameter is ignored. 
PATERN 
Velocity profile of moving tool.  If the velocity is user defined by
*BOUNDARY_PRESCRIBED_RIGID_BODY, PATERN is ignored.
EQ.1: Ramped velocity profile 
EQ.2: Smooth velocity curve 
VX, VY, VZ 
Vector  components  defining 
the  direction  of 
movement.  The default direction is defined by VID. 
the  punch
VID 
Vector  ID  defining  the  direction  of  the  punch  movement.    This
variable  overrides  the  vector  components  (VX,  VY,  VZ).    If  VID
and  (VX,  VY,  VZ)  are  undefined, the  punch  is  assumed  to  move 
in the negative z-direction. 
AMAX 
The maximum allowable acceleration. 
LVLADA 
Maximum adaptive level. 
SIZEADA 
Minimum element size permitted in the adaptive mesh. 
TIMSADA 
Total number of adaptive steps during the forming simulation. 
D3PLT 
The total number of output states in the D3PLOT database.
*CONTROL_FORMING_TEMPLATE 
UNIT 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Mass 
Ton 
Gm 
Gm 
Gm 
Gm 
Kg 
Kg 
Kg 
Kg 
Kg 
Length  Mm  Mm  Mm 
Cm 
Cm  Mm 
Cm 
Cm 
Cm 
Time 
Force 
S 
N 
Ms 
S 
Us 
S 
Ms 
Us 
Ms 
S 
N 
𝜇N 
1e7N  Dyne  KN 
1e10N 1e4N  1e-
2N 
m 
S 
N 
Table 12-58.  Available units for metal stamping simulation. 
About IDTEMP: 
When the variable IDTEMP is set to 1, it represents a 3-piece draw in air, as shown in 
Figure 12-55.  When IDTEMP is set to 2, a 3-piece toggle draw is assumed, Figure 12-56.  
For IDTEMP of 1 or 2, LS-DYNA will automatically position the tools and minimize the 
punch  travel  (step  a),  calculate  the  binder  and  punch  travel  based  on  the  blank 
thickness and the home gap (step b), set the termination time based on step (a) and (b), 
define the rigid body motion of the tooling, establish all the contacts between the blank 
and rigid tools, and, select all necessary control parameters.  
When  IDTEMP  is  set  to  3,  a  4-piece  stretch  draw  shown  in  Figure  12-57  will  be 
followed.  The die action goes as follows: after upper binder moves down to fully close 
with lower binder, both pieces move together down a certain distance (usually ~50mm) 
to “pull” the blank  “over” the lower die, then upper punch closes with the lower die, 
finally the binders  move down together to their home position. 
Both toggle draw and 4-piece stretch draw are called “double action” processes which 
suffer from a slower stamping speed.  As the metric of “hits per minute” (or “parts per 
minute”)  becomes  a  stamping  industry  benchmark  for  efficiency,  these  types  of  draw 
are  becoming  less  popular  (especially  the  4-piece  stretch  draw).    Nevertheless,  they 
remain  important  stamping  processes  for  controlling  wrinkles  in  difficult-to-form 
panels such as lift gate inners, door inners and floor pans.  These two processes are also 
used  in  situation  where  deep  drawn  panels  require  draw  depth  of  over  250mm,  the 
usual limit for automatic transfer presses. 
For  all  the  above  IDTEMP  values,  users  do  not  need  to  define  additional  keywords, 
such  as  *PART,  *CONTROL,  *SECTION,  *MAT_…,  *CONTACT_…  (drawbead 
definition is an exception), and, *BOUNDARY_PRESCRIPTION_RIGID, etc.  If any such 
keyword is defined, automatic default settings will be overridden.
When  IDTEMP  is  set  to  4,  springback  Simulation  will  be  conducted.    The  only 
additional  keyword,  *BOUNDARY_SPC_…  is  needed  to  specify  the  constraints  in  the 
input deck. 
When IDTEMP is set to 5, a trimming operation will be performed.  The only additional 
keyword,  *DEFINE_CURVE_TRIM,  is  needed  to  specify  the  trim  curves  in  the  input 
deck. 
Revision information: 
This feature is available starting in Revision 45901 and later releases.
*CONTROL_FORMING_TIPPING 
Purpose:    This  keyword  is  developed  to  reorient  or  reposition  a  part  between  the 
stamping dies.  In stamping line die simulation, panel tipping and translation between 
the die stations are frequently required.  Typically such transformation involves only a 
small amount of rotations, e.g. < 15 degrees; and some large amounts of translation.  For 
example, there could be a tipping angle of 10 degree along Y-axis and a translation of 
2000 mm along the X-axis between the current trimming die and next flanging die. 
Card Set.  For each rotated or translated part or set add a Tipping Card plus NMOVE 
Move Cards.  The data set for this keyword ends at the next keyword (“*”) card. 
Tipping Card.  Specify a part or set ID to be tipped. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID/SID 
ITYPE 
ISTRAIN 
IFSTRSS 
NMOVE 
Type 
I 
I 
Default 
none 
none 
I 
0 
I 
0 
I 
0 
Move Card (Rot).  Format when first entry, ROT/TRAN, is set to 1. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  ROT/TRAN 
V11 
V12 
V13 
X01 
Y01 
Z01 
DISTA1 
Type 
I 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0
Move Card (Trans).  Format when first entry, ROT/TRAN, is set to 2. 
5 
6 
7 
8 
  Card 2 
1 
2 
Variable  ROT/TRAN 
DX 
Type 
I 
F 
3 
DY 
F 
4 
DZ 
F 
Default 
none 
0.0 
0.0 
0.0 
  VARIABLE   
PID/SID 
DESCRIPTION
Part  ID  or  part  set  ID  of  part(s)  that  requires  tipping  and/or
translation. 
ITYPE 
Part ID or part set ID indicator: 
EQ.1: PID means part ID, 
EQ.2: PID/SID means part set ID. 
ISTRAIN 
Strain tensors inclusion option: 
EQ.1: include in tipping/translation. 
ISTRESS 
Stress tensors inclusion option: 
EQ.1: include in tipping/translation. 
NMOVE 
Total  number  of  tipping  and  translation  intended  with  this
keyword. 
ROT/TRAN 
Transformation type: 
EQ.1: rotation, 
EQ.2: translation. 
V11, V12, 
V13 
X01, Y01, 
Z01 
Vector components of an axis about which tipping is performed. 
X, Y and Z coordinates of a point through which the tipping axis
passes. 
DSITA 
Tipping angle in degree. 
DX, DY, DZ 
Translation distances along global X-axis, Y-axis and Z-axis.
*CONTROL_FORMING_TIPPING 
1.  Keyword *INCLUDE can be used to include the file to be tipped or translated.  
2.  Tipping angle DISTA1 is defined in degree.  Signs of the tipping angles follow 
the “right hand rule”. 
3.  An example of the keyword is included below, to tip a part +23.0 degrees, -31.0 
degrees,  and  +8.0  degrees  about  X-,  Y-,  and  Z-axis,  respectively  and  passing 
through the origin; and to translate the part 12.0mm, -6.0mm and 91.0mm along 
X, Y, and Z axis, respectively. 
*INCLUDE 
trimmedpart.dynain 
*CONTROL_FORMING_TIPPING 
$ PID/PSID     ITYPE   ISTRAIN    ISTRSS     NMOVE 
         1         0         1         1         4 
$ ROT/TRAN       V11       V12       V13       X01       y01       z01    DSITA1 
         1     1.000  0.000000     0.000     0.000     0.000     0.000      23.0 
$ ROT/TRAN       V21       V22       V23       X21       y21       z21    DSITA2 
         1     0.000  1.000000     0.000     0.000     0.000     0.000     -31.0 
$ ROT/TRAN       V31       V32       V33       X31       y31       z31    DSITA3 
         1  0.000000     0.000     1.000     0.000     0.000     0.000       8.0 
$ ROT/TRAN        DX        DY        DZ    
2     12.0      -6.0      91.0 
Revision Information: 
This feature is available starting in LS-DYNA Revision 53448, with major updates from 
Revision  80261.    It  is  also  available  in  LS-PrePost4.0  eZSetup  for  metal  forming 
application (http://ftp.lstc.com/anonymous/outgoing/lsprepost/4.0/metalforming/).
*CONTROL_FORMING_TOLERANC 
Purpose:  This keyword utilizes a smoothing algorithm to reduce the output noise of the 
strain  ratio  β  (minor  strain/major  strain)  in  calculating  the  Formability  Index  (F.I.), 
which predicts sheet metal failure under nonlinear strain paths frequently occurred in 
metal forming application.  This keyword must be used together with the NLP option in 
and for *MAT_036 and *MAT_037 only; and applies to shell elements only.  This feature 
is jointly developed with the Ford Motor Company. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  DT/CYCLE  WEIGHT  OUTPUT 
Type 
F 
F 
Default 
none 
none 
I 
0 
  VARIABLE   
DESCRIPTION
DT/CYCLE 
Flag for output option (time interval or cycle number). 
DT/CYCLE.LT.0:  The  absolute  value  is  the  time  interval 
between outputs. 
DT/CYCLE.GT.0:  Cycle numbers between outputs. 
WEIGHT 
Coefficient α in equation below. 
OUTPUT 
Output  flag.    When  OUTPUT  is  set  to  1,  information  such  as
integration  point,  element  ID,  time,  strain  ratio  β,  major  and 
minor  strains  will  be  output  to  the  “.o”  file  (a  scratch  file  from 
batch queue run). 
Remarks: 
The incremental change of in-plane major and minor strains are smoothed according to 
the following formula: 
∆𝜖1(𝑛−1) ∗ (1 − 𝛼) + 𝑑𝜖1(𝑛) ∗ 𝛼 
∆𝜖2(𝑛−1) ∗ (1 − 𝛼) + 𝑑𝜖2(𝑛) ∗ 𝛼 
where, 𝑑𝜖1(𝑛) and 𝑑𝜖2(𝑛) are incremental changes of 𝜖1 and 𝜖2  in the current time step n,  
∆𝜖1(𝑛−1) and ∆𝜖2(𝑛−1) are incremental changes of 𝜖1 and 𝜖2 in the previous time step n-
1.  The weighting coefficient 𝛼 regulates the smoothness of the incremental changes in 
𝜖1 and 𝜖2.
Strain ratio 𝛽 results from smoothed incremental major and minor strains and stored in 
history variable #2 along with additional information  in “.o” 
file  if  running  in  a  batch  queueing  system,  or  directly  dumped  onto  the  screen  if 
running in an interactive window. 
𝛽 =
∆𝜖2(𝑛−1) ∗ (1 − 𝛼) + 𝑑𝜖2(𝑛) ∗ 𝛼
∆𝜖1(𝑛−1) ∗ (1 − 𝛼) + 𝑑𝜖1(𝑛) ∗ 𝛼
The upper limit of 𝛽 is set at 1.0 while the lower limit is: 
where 𝑟 ̅ is the anisotropic parameter: 
−
𝑟 ̅
1 + 𝑟 ̅
𝑟 ̅ =
𝑟0 + 2𝑟45 + 𝑟90
where  𝑟0,  𝑟45  and  𝑟90  are  Lankford  parameter  in  the  rolling,  diagonal  and  transverse 
direction, respectively. 
The  keyword  usage  is  shown  in  the  following  partial  input  deck,  where  *MAT_3-
PARAMETER_BARLAT_NLP  is  used.    Note  NEIPS  is  set  at  3  for  output  of  3  history 
variables that include formability index (F.I.), strain ratio 𝛽 and effective plastic strain 𝜀̅. 
*KEYWORD 
*INCLUDE_TRIM 
sim_trimming.dynain 
⋮  
*DATABASE_EXTENT_BINARY 
$    NEIPH     NEIPS    MAXINT    STRFLG    SIGFLG    EPSFLG    RLTFLG    ENGFLG 
                   3      &nip         1 
⋮  
*PARAMETER_EXPRESSION 
R d3plot   endtime/1000.0 
R nt       -1.0*d3plot 
... 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*CONTROL_FORMING_TOLERANC 
$ DT/CYCLE    WEIGHT    OUTPUT 
       &nt      0.15         1 
*MAT_3-PARAMETER_BARLAT_NLP 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
$      MID        RO         E        PR        HR 
        13   7.8E-09  2.07E+05      0.30     3.000 
$        M       R00       R45       R90      LCID 
     6.000     1.200     1.450     1.090        99 
$     AOPT         C         P     VLCID                           NLP 
     2.000                                                         200 
$                                      A1        A2        A3 
                                    1.000     0.000     0.000 
$       V1        V2        V3         D1        D2        D3 
                                    0.000     1.000     0.000 
*DEFINE_CURVE 
      200 
$FORM LIMIT DIAGRAM 
             -0.7000              0.8309 
             -0.4500              0.6805 
             -0.2500              0.5081
0.0000              0.2479 
              0.2000              0.3487 
              0.4000              0.3845 
*DEFINE_CURVE  
        99  
     0.000000000E+00     0.166100006E+03  
     0.579999993E-02     0.189110001E+03  
     0.124000004E-01     0.204789993E+03  
     0.190999992E-01     0.218520004E+03  
     0.255999994E-01     0.230580002E+03  
            ⋮                    ⋮ 
     0.100000000E+01     0.512053406E+03 
... 
*END 
As  shown  in  Figure  12-59,  beta  smoothed  using  smoothing  algorithm  is  much  better 
than  unsmoothed  one.    Most  importantly,  a  plot  of  strain  path  (Figure  12-60)  in  the 
traditional FLD space (𝜖1 vs. 𝜖2) confirms the terminal beta is approximately 0.9, which 
is much closer to the smoothed beta value (Figure 12-59) at the end of the simulation. 
Output 
items 
Columns 
IP # 
Element ID 
Time 
β 
𝜖1 
𝜖2 
1st to 8th  
9th to18th 
19th to 29th  30th to 40th  41th to 51th  52th to 62th
Table  12-2.    “.o”  file  output  information  and  positions.    Note  only  the  mid-IP 
information are output. 
Revision Information: 
Revision history information is listed below.  Output information in “.o” file currently 
applies to SMP and 1 CPU MPP only. 
1)LS-DYNA Revision 84159: β smoothing is enabled for *MAT_036. 
2)Revision 110928: β smoothing is enabled for *MAT_037.
1.2
0.8
0.4
0.0
-0.4
0.0
Unsmoothed beta
Smoothed beta
0.005
0.010
0.015
0.020
Time (seconds)
Figure 12-59.  Effect of smoothing on strain ration β. 
Terminal trendline
y=1.11x+0.0651, β=0.9
0.14
0.12
0.10
0.08
0.06
0.04
0.02
0.00
0.00
0.02
0.04
0.06
0.08
0.10
0.12
0.14
Minor true strain
Figure 12-60.  Strain path and terminal strain ratio β value.

*CONTROL_FORMING_TRAVEL 
Purpose:  This keyword allows user to define tool travel for each phase in a  stamping 
process simulation.  The entire simulation process can be divided into multiple phases 
corresponding  to the  steps  of  an  actual  metal  forming  process.    This  keyword  is  to  be 
used  for  tools  that  are  pre-positioned  above  the  sheet  blank  (or  below  the  blank)  and 
ready  for  forming.    For  tools  that  are  pre-positioned  at  their  home  positions,  *CON-
TROL_FORMING_TRAVEL  should  be  used.    This  keyword  is  used  together  with 
*CONTROL_FORMING_USER. 
NOTE:  This  option  has  been  deprecated  in  favor  of  *CON-
TROL_FORMING_AUTOPOSITION_PARAME-
TER). 
Define  Travel  Cards.    Repeat  Card  as  many  times  as  needed  to  define  travels  in 
multiple phases.  The next “*” card terminates the input. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
VID 
TRAVEL 
TARGET 
GAP 
PHASE 
FOLLOW 
Type 
I 
I 
F 
I 
F 
I 
I 
Default 
none 
none 
none 
none 
1.0t 
none 
none 
  VARIABLE   
DESCRIPTION
PID 
VID 
TRAVEL 
TARGET 
GAP 
Part ID of a stamping tool, as defined in *PART. 
Vector  ID  defining  the  direction  of  travel  for  the  tool  defined  by 
the PID. 
The  distance  in  which  the  tool  will  be  traveled  to  complete
forming  in  the  direction  specified  by  the  VID.    If  TRAVEL  is
defined, it is unnecessary to define TARGET. 
Target tool PID, as defined in *PART.  The tool (defined by PID) 
will  be  traveled  to  where  the  TARGET  tool  is  to  complete
forming. 
The minimum distance between the tool (PID) and TARGET tool
at the home position (forming complete).  The GAP is by default
the sheet blank thickness “t”.
DESCRIPTION
Phase number, starting sequentially from 1.  For example, phase 1
is the binder closing, and phase 2 is the drawing operation. 
Part ID of a stamping tool to be followed by the tool (PID).  When
this  variable  is  defined,  the  distance  between  the  tool  (PID)  and 
part  ID  defined  by  FOLLOW,  will  remain  constant  during  the
phase. 
  VARIABLE   
PHASE 
FOLLOW 
Remarks: 
FOLLOW can be used to reduce total simulation time.  For example, in a toggle draw, 
the  upper  punch  travels  together  with  the  upper  binder  during  binder  closing  phase, 
thus  reducing  the  upper  travel  distance  during  the  draw,  shortening  the  overall 
termination time. 
An example is provided in manual pages under *CONTROL_FORMING_USER.
*CONTROL_FORMING_TRIM_MERGE 
Purpose:    This  feature  allows  for  automatic  close  of  any  open  trim  loop  curve  for  a 
successful trimming simulation.  Previously, sheet metal trimming would fail if a trim 
curve  does  not  form  a  closed  loop.    This  keyword  is  used  together  with  *DEFINE_-
CURVE_TRIM,  *ELEMENT_TRIM,  *DEFINE_VECTOR,  *CONTROL_ADAPTIVE_-
CURVE, *CONTROL_CHECK_SHELL, and applies to shell elements only. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IMERGE 
GAPM 
Type 
Default 
I 
1 
F 
0.0 
  VARIABLE   
DESCRIPTION
IMERGE 
Activation flag.  Set to ‘1’ (default) to activate this feature. 
GAPM 
Gap distance between two open ends of a trim loop curve in the
model.  If the gap is smaller than GAPM, the two open ends of a
trim curve will be closed automatically. 
Remarks: 
1. 
If  multiple  open  trim  loop  curves exist,  GAPM  should  be  set  to  a value  larger 
than any of the gap distances of any trim curves in the trim model. 
2.  An example provided below shows that for both 3D (#90905) and 2D trim curve 
(#90907), each with an open gap of 2.3 and 2.38mm, respectively.  An automatic 
merge operation is being performed with the GAPM set at 2.39 mm.  Since this 
set  value  is  larger  than  both  gaps  in  the  model,  trimming  will  automatically 
close the gap for both curves and to form two closed-loop curves for a success-
ful trim.  In Figure 12-61, two different 2D trimming results are illustrated with 
GAPM of 2.39 (successful) as well as 2.37 (fail). 
*KEYWORD 
*INCLUDE_TRIM 
drawn2.dynain 
⋮  
*CONTROL_ADAPTIVE_CURVE 
$    IDSET     ITYPE         N      SMIN 
   &blksid         2         3       0.6
GAP=2.38 mm
Trim vector
2D trim with GAPM=2.39
Trim loop curve
GAP=2.38 mm
2D trim with GAPM=2.37
Figure 12-61.  A 2D trimming with different GAPM values. 
*CONTROL_CHECK_SHELL 
$     PSID    IFAUTO    CONVEX      ADPT    ARATIO     ANGLE      SMIN 
  &blksid1         1         1         1  0.250000150.000000  0.000000 
*DEFINE_CURVE_TRIM_3D 
$#    tcid    tctype      tflg      tdir     tctol      toln    nseed1    
nseed2 
     90907         2         1         0  1.250000  2.500000         0         
0 
sim_trimline_03.igs 
*DEFINE_CURVE_TRIM_NEW 
$#    tcid    tctype      tflg      tdir     tctol      toln    nseed1    
nseed2 
     90905         2         0         2  1.250000  1.000000         0         
0 
$# filename 
sim_trimline_02.igs 
*DEFINE_VECTOR_TITLE 
vector for Trim curve 90905 
$#     vid        xt        yt        zt        xh        yh        zh       
cid
2     0.000     0.000     0.000 -0.170000  0.950000 -0.260000         
0 
*ELEMENT_TRIM 
&blksid 
*DEFINE_TRIM_SEED_POINT_COORDINATES 
$ NSEED,X1,Y1,Z1,X2,Y2,Z2 
1,&seedx,&seedy,&seedz 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+---
-8 
*CONTROL_FORMING_TRIM_MERGE 
$   IMERGE      GAPM 
         1      2.39 
$ Note that the 3D trim curve has a gap of 2.3 and the 2D trim curve has a gap 
of 2.38 
*END 
3.  This feature is available starting in LS-DYNA Revision 84098.
*CONTROL_FORMING_TRIMMING 
Purpose:  Define a part subset to be trimmed by *DEFINE_CURVE_TRIM.  This feature 
is intended for metal forming simulation.  Currently trimming is enabled on 2D and 3D 
trimming of shell elements, 3D solid element, adaptive sandwiched parts (one layer of 
solid elements with top and bottom layers of shell elements), non-adaptive sandwiched 
parts  (multiple  layers  of  solid  elements  with  top  and  bottom  layers  of  shell  elements), 
and  2-D  trimming  of  thick  shell  elements  (TSHELL).    Note  it  is  not  applicable  to 
axisymmetric  solids  or  2D  plane  strain/stress  elements.    For  details,  see  *DEFINE_-
CURVE_TRIM. 
NOTE:  Before  revision  87566  this  card  was  called  ELE-
MENT_TRIM. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PSID 
ITYP 
Type 
I 
Default 
none 
I 
0 
  VARIABLE   
DESCRIPTION
Part set ID for trimming, see *SET_PART. 
Activation flag for sandwiched parts (laminates) trimming: 
ITYP.EQ.0: Trimming for solid elements. 
ITYP.EQ.1: Trimming for laminates. 
PSID 
ITYP 
Remarks: 
This keyword is used together with *DEFINE_CURVE_TRIM to trim the parts defined 
in PSID at time zero, i.e., before any stamping process simulation begins.  Elements in 
the part set will be automatically trimmed in the defined direction if they intersect the 
trim curves.  See examples in keyword section *DEFINE_CURVE_TRIM.
*CONTROL_FORMING_TRIMMING 
1.  Revision  87566:  *ELEMENT_TRIM  was  changed  to  the  current  name  *CON-
TROL_FORMING_TRIMING. 
2.  Revision  95745:  *CONTROL_FORMING_TRIMING  was  changed  to  *CON-
TROL_FORMING_TRIMMING. 
3.  Revision 92088: 2-D trimming of solid elements is implemented. 
4.  Revision 92289: 2-D and 3-D trimming of laminates (ITYP) is added. 
5.  Revision 93467: 3-D trimming of solid elements is added. 
6.  Latter Revisions may incorporate more improvements and are suggested to be 
used for trimming.
*CONTROL_FORMING_UNFLANGING_{OPTION} 
Available options include: 
<BLANK> 
OUTPUT 
Purpose:  The keyword unfolds flanges of a deformable blank onto a rigid tooling mesh 
using  an  implicit  statics  solver.    This  is  typically  used  in  trim  line  unfolding  during  a 
stamping  die  development  process.    The  option  OUTPUT  must  be  used  together  with 
*CONTROL_FORMING_UNFLANGING  to  get  the  modified  trim  curves.    Other 
keywords  related  to  blank  size  development  are,  *CONTROL_FORMING_ONESTEP, 
and *INTERFACE_BLANKSIZE_DEVELOPMENT. 
Card 1 for no option, <BLANK>: 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  NOPTION 
DVID 
NUNBEND STFBEND STFCNT 
IFLIMIT 
DIST 
ILINEAR 
Type 
I 
I 
I 
F 
F 
I 
F 
Default 
none 
N/A 
none 
none 
none 
none 
none 
I 
2 
Card 2 for no option, <BLANK>: 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NB1 
NB2 
NB3 
CHARLEN NDOUTER
Type 
I 
I 
I 
F 
I 
Default 
none 
none 
none 
150.0 
none
*CONTROL_FORMING_UNFLANGING 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
THMX 
THMN 
EPSMX 
Type 
I 
I 
I 
Default 
1020 
0.0 
1020 
  VARIABLE   
DESCRIPTION
NOPTION 
Flag to turn on an unfolding simulation: 
EQ.1: Activate the unfolding simulation program. 
DVID 
This variable is currently not being used. 
NUNBEND 
Estimated number of unbending, ranging from 10 to 100. 
STFBEND 
Unflanging stiffness, ranging from 0.1 to 10.0. 
STFCNT 
Normal stiffness, ranging from 0.1 to 10.0. 
IFLIMIT 
DIST 
Iteration  limit  for  the  first  phase  of  unfolding,  typically  ranging
from 11 to 400. 
Distance  tolerance  for  auto-SPC  along  flange  root.    DIST  (Figure 
12-63) is usually slightly more than ½ of the flange thickness.  This 
field must be left blank for ILINEAR = 2.  Also, nodes along the root 
can be directly positioned on the rigid body surface (addendum),
leaving a DIST of zero (Figure 12-63). 
ILINEAR 
Unfolding algorithm selection flag: 
EQ.0:  Nonlinear unfolding. 
EQ.1:  Linear unfolding. 
EQ.2:  A  hybrid  unfolding  method  (Revision  87100  and  later).
The curved 3D meshes of the flange will first be mapped
onto the tooling surface to be used as a starting porting
for nonlinear iterations; unfolding completes when force 
balance is reached. (recommended).
VARIABLE   
NB1 
NB2 
NB3 
CHARLEN 
NDOUTER 
THMX 
DESCRIPTION
The start node ID (Figure 12-64) on a flange root boundary (fixed 
end  of  the  flange,  see  Figures  12-63  and  12-64).    For  closed-loop 
flange root boundary, only this parameter needs to be defined; for
open-loop flange root boundary, define this parameter as well as
NB2  and  NB3.    The  solver  will  automatically  identify  and
automatically  impose  the  necessary  boundary  constraints  on  all
the  nodes  along  the  entire  three-dimensional  flange  root 
boundary. 
The  ID  of  a  node  in  the  middle  of  the  flange  root  boundary,  see
Figure  12-64.    Define  this  parameter  for  open-loop  flange  root 
boundary only. 
The  end  node  ID  on  a  flange  root  boundary.    Define  this
parameter for open-loop flange root boundary only.  The “path” 
formed  by  NB1,  NB2  and  NB3  can  be  in  any  direction,  meaning
NB1 and NB3 (Figure 12-64) can be interchangeable. 
Maximum  flange  height  (Figure  12-64)  to  limit  the  search  region 
for the boundary nodes along the flange root.  This value should
be set bigger than the longest width (height) of the flange; and it
is  needed  in  some  cases.    This  parameter  is  now  automatically
calculated as of Revision 92860. 
A node ID on the outer flange (free end of the flange) boundary.
This node helps search of nodes along the flange root, especially 
when holes are present in the flange area, see Figure 12-64. 
Maximum  thickness  beyond  which  elements  are  deleted;  this  is
useful  in  removing  wrinkling  areas  of  the  flange  (shrink  flange). 
Modified,  unfolded  flange  outlines  based  on  this  parameter  are
stored  in  a  file  called  “trimcurve_upd.k”,  written  using  the  *DE-
FINE_CURVE_TRIM_3D; keyword.  The modified flanges (before 
unfolding) are in a keyword file called “mdfiedflangedpart.k”; and 
the  unmodified  flange  (unfolded)  is  in  “trimcurve_nmd.k”,  also 
written  using  keyword  *DEFINE_CURVE_TRIM_3D.    See  the 
example  in  Figure  12-64  for  an  explanation.    Currently  the 
modified  flange  and  curves  are  not  smooth,  which  will  be
improved in the future.  To convert between *DEFINE_CURVE_-
TRIM_3D  and  IGES  format,  refer  to  Figures  in  *INTERFACE_-
BLANKSIZE.
THMN 
*CONTROL_FORMING_UNFLANGING 
DESCRIPTION
Minimum  thickness  below  which  elements  are  deleted;  this  is
useful  in  removing  overly  thinned  areas  of  the  flange  (stretch
flange).    Updated  flange  information  based  on  this  parameter  is
stored in files listed above. 
EPSMX 
Maximum  effective  plastic  strain  beyond  which  elements  are
deleted; this is useful in removing flange areas with high effective 
plastic strains (stretch flange).  Updated flange information based
on this parameter is stored in files listed above. 
Introduction: 
Unfolding  of  flanges  is  one  of  the  first  steps  in  a  stamping  die  development  process.  
Immediately  after  tipping,  binder  and  addendums  are  built  for  unfolding  of  flanges.  
According  to  process  considerations  (trim  conditions,  draw  depth,  and  material 
utilization, etc.), the addendums are built either in parallel or perpendicular to the draw 
die  axis,  tangentially  off  the  main  surface  off  the  breakline  ,  or  any 
combinations of the three scenarios.  Trim lines are developed by unfolding the flanges 
in finished (hemmed or flanged) position onto these addendums.  Addendum length in 
some areas may have to be adjusted to accommodate the unfolded trim lines.  Trim line 
development  is  very  critical  in  hard  tool  development.    Inaccurate  trim  lines  lead  to 
trim  die  rework,  result  in  many  hours  of  re-welding,  re-machining  and  re-spotting  of 
trim die components. 
Input and output: 
The inputs for the keyword are: 
1.  blank or flanges in the finished configuration, and, 
2. 
the draw die surface in mesh. 
Meshes for flanges should of a quality similar to the blank mesh one would build for a 
forming simulation.  In LS-PrePost 4.0, this kind of mesh can be created using Mesh → 
Automesh  →  Size.    Element  formulation  16  with  NIP  set  to  5  is  recommended  for  the 
blank.    The  output  results,  in  terms  of  unfolding  steps  and  final  unfolded  flanges,  are 
stored in the d3plot files.  LS-PrePost 4.0 function of Curve → Spline → From Mesh → By 
part can be used to create unfolded flange/trim curves from the unfolded flanges.  Since 
the  program  uses  an  implicit  statics  solver,  the  double  precision  version  of  LS-DYNA 
must be used.
Other modeling guidelines: 
1.  All addendum and flanges need to be oriented as if they are in a draw position, 
with the drawing axis parallel to the global Z-axis; specifically the flanges need 
to be on top of the addendum, as noted in Figures 12-62, 12-63 and 12-64. 
2.  Normals  of  the  to-be-unfolded  flange  side  and  tool  surface  side  must  be 
consistent  and  must  face  against  each  other  when  the  flange  is  unfolded,  see 
Figure 12-64. 
3.  Holes in the blank are allowed only for ILINEAR = 2. 
4.  Adaptive re-meshing is not supported. 
5.  To-be-unfolded  flange  and  tool  meshes  must  not  share  the  same  nodes.    This 
can be easily done using the mesh detaching feature under EleTol → DetEle in 
LS-PrePost. 
6.  Meshes  of  the  flange  part  and  rigid  tool  can  slightly  overlap  each  other,  but 
large amounts of overlap (area of flange already on addendum surface) is not 
allowed.  In LS-PrePost the EleTol → PtTrim feature can trim off the overlapped 
flange  portion.    The  curves  used  for  the  trimming  can  be  obtained  from  the 
flange  tangent  curves  on  the  addendum  (which  has  a  more  regulated  mesh 
pattern) using LS-PrePost’s Curve → Spline → Method From Mesh → By Edge 
→ Prop feature with appropriate angle definition.  Furthermore, any holes are 
not allowed in the overlapping area. 
7. 
*CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE 
should  be 
used  for  the  contact  between  the  blank  and  tool.    Negative  tool  offsets  on  the 
*CONTACT_… keyword is not supported. 
8.  The  rigid  tool  (total  fixed  in  *MAT_020)  must  be  larger  than  the  unfolded 
flanges, especially along symmetric lines.  This may be obvious, nevertheless it 
is sometimes overlooked. 
9.  Nodes along the flange root are automatically fixed by defining NB1, NB2 and 
NB3, as shown in Figure 12-64. 
10.  No “zigzag” along the flange root boundary, meaning that the boundary along 
the  flange  root  must  be  smooth.    This  restriction  is  removed  as  of  Revision 
92727. 
11.  Symmetric boundary conditions are supported. 
12.  Thickness  and  effective  plastic  strain  are  stored  in  a  file  “unflanginfo.out”, 
which can be plotted in LS-PrePost 4.0, see Figure 12-64.
*CONTROL_FORMING_UNFLANGING 
A partial input deck is provided below for flange unfolding of a fender outer, modified 
from the original NCAC Taurus model.  Shown in Figure 12-62 are the progressions of 
the  unfolding  process,  where  the  finished  flanges  are  to  be  unfolded  onto  the 
addendum (rigid body).  A section view of the same unfolding before and after is found 
in Figure 12-63.  ILINEAR is set at 2 while DIST is left blank.  Total numbers of elements 
are 1251 on the blank and 6600 on the tooling.  It took less than 3 minutes on an 8 CPU 
(SMP)  machine.    Note  that  additional  keywords,  such  as  *CONTROL_IMPLICIT_-
FORMING,  etc.    are  used.    Termination  criterion  is  set  using  the  variable  DELTAU  in 
*CONTROL_IMPLICIT_TERMINATION.    Termination  is  reached  when  the  relative 
displacement ratio criterion is met, as indicated in the messag file.  Termination time of 
10.0  (steps)  is  sufficient  for  most  cases,  but  may  need  to  be  extended  in  some  cases  to 
satisfy the DELTAU in some cases. 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*KEYWORD 
*INCLUDE 
toolblankmesh.k 
*CONTROL_FORMING_UNFLANGING 
$  NOPTION      DVID   NUNBEND   STFBEND    STFCNT   IFLIMIT      DIST   ILINEAR 
         1                 100       0.2      15.0       400                   2 
$      NB1       NB2       NB3   CHARLEN   NDOUTER 
       321       451       322      60.0      6245 
*CONTROL_IMPLICIT_FORMING 
1 
*CONTROL_IMPLICIT_TERMINATION 
$   DELTAU 
$ set between 0.0005~0.001 
    0.0005 
*CONTROL_IMPLICIT_GENERAL 
$   IMFLAG       DT0 
         1     .1000 
*CONTROL_IMPLICIT_SOLUTION 
$  NSLOLVR    ILIMIT    MAXREF     DCTOL     ECTOL     RCTOL     LSTOL 
         2         2      1100     0.100     1.e20     1.e20        
$    dnorm   divflag   inistif 
         0         2         0         1                   1             
*PARAMETER 
R ENDTIME       10.0 
I elform          16 
I nip              5 
R bthick         1.0 
*PARAMETER_EXPRESSION 
R D3PLOTS    ENDTIME/60.0 
*CONTROL_TERMINATION 
&ENDTIME 
*DATABASE_BINARY_D3PLOT 
&D3PLOTS 
*CONTROL_RIGID... 
*CONTROL_HOURGLASS... 
*CONTROL_BULK_VISCOSITY... 
*CONTROL_SHELL... 
*CONTROL_CONTACT 
$   SLSFAC    RWPNAL    ISLCHK    SHLTHK    PENOPT    THKCHG     ORIEN 
      0.01       0.0         2         1         4         0         4 
$   USRSTR    USRFAC     NSBCS    INTERM     XPENE     SSTHK      ECDT   TIEDPRJ 
         0         0        10         0       2.0         0 
*CONTROL_ENERGY... 
*CONTROL_ACCURACY...
*DATABASE_EXTENT_BINARY... 
*SECTION_SHELL_TITLE 
BLANK/FLANGE thickness and elform/nip specs. 
&blksec      &elform     0.833      &nip       1.0 
&bthick,&bthick,&bthick,&bthick 
*PART... 
*MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLASTIC... 
*MAT_RIGID... 
*CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE 
$     SSID      MSID     SSTYP     MSTYP    SBOXID    MBOXID       SPR       MPR 
   &blkpid   &diepid         3         3                            
$       FS        FD        DC        VC       VDC    PENCHK        BT        DT 
     0.125       0.0       0.0       0.0      20.0         0       0.0 1.000E+20 
$      SFS       SFM       SST       MST      SFST      SFMT       FSF       VSF 
       1.0       1.0       0.0    
$     SOFT    SOFSCL    LCIDAB    MAXPAR    PENTOL     DEPTH     BSORT    FRCFRQ 
         0 
$   PENMAX    THKOPT    SHLTHK     SNLOG      ISYM     I2D3D    SLDTHK    SLDSTF 
$     IGAP    IGNORE    DPRFAC    DTSTIF                        FLANGL 
         2 
*END 
In  Figure  12-64  (top),  with  THMN  set  at  0.4mm,  the  stretch  flange  area  of  the  corner, 
which has thickness less than 0.4mm, is removed; and the modified flange outlines are 
created accordingly (bottom).  The partial input used is listed below. 
*CONTROL_FORMING_UNFLANGING 
$  NOPTION      DVID   NUNBEND   STFBEND    STFCNT   IFLIMIT      DIST   ILINEAR 
         1                 100       0.2      15.0       400                   2 
$      NB1       NB2       NB3   CHARLEN   NDOUTER 
       321       451       322      60.0      6245 
*CONTROL_FORMING_UNFLANGING 
$     THMX      THMN     EPSMX 
                 0.4 
Revision information: 
The  feature  is  available  in  double  precision  SMP,  and  starting  in  LS-DYNA  Revision 
73190.  Revision information is listed below for various parameters and features: 
1. 
ILINEAR = 2: Revision 87100. 
2.  NDOUTER: Revision 87318. 
3.  CHARLEN: Revision 87210. 
4.  NB1, NB2, NB3: Revision 87100. 
5.  Option OUTPUT: Revision 86943. 
6.  Holes allowed: Revision 87167. 
7.  File “mdfiedflangedpart”: Revision 87105.
8.  Symmetric boundary condition: Revision 88359. 
9.  CHARLEN automatically calculated: Revision 92860. 
10.  “Zigzag” flange root boundary allowed: Revision 92727.
Finished flanges
30% 
unfolded
Flanges must be on top of the 
addendum in the draw position
Addendum
60% 
unfolded
Unfolded flanges
100% 
unfolded
  Figure 12-62.  Flange unfolding progression of a fender outer (original model 
courtesy of NCAC at George Washington University).
Addendum
Finished (incoming) 
flanges
Unfolded flanges
Flange root (fixed end)
Free end of the flange
Flanges must be on top of the 
addendum in the draw position
DIST
  Figure 12-63.  A section view showing flange unfolding before and after.
Thickness contour
min=0.2257 
max=0.8533
Thickness (mm)
Holes are allowed
Thickness in the 
dark blue area less 
than 0.4mm, at 
which THMN is set.
Flange normals
Addendum normals
0.85
0.79
0.73
0.67
0.60
0.54
0.48
0.41
0.35
0.29
 0.23
Addendum surface
Flange before unfolding
Unfolded flange.  Thickness and 
effective plastic strain contour are 
stored in a file "unflanginfo.out"
NB3
Flange must be on top of the 
addendum in the draw position
CHARLEN
NDOUTER
NB2
Flange root 
boundary (fixed) 
NB1 - define this only for a closed-loop 
boundary; define all three (NB1, NB2, 
NB3) for an open-loop boundary.
Original flange is modified based on 
THMN=0.4 and the mesh is stored in a file 
"mdfiedflangedpart.k".  Boundary curves 
can be created using  LSPP4.0 under 
Curve/Spline/From mesh/by part.
Modified boundary curves on 
unfolded flange are stored in a file 
"trimcurve_upd.k"; original boundary 
curves (without the corner cutout) is 
in "trimcurve_nmd.k". 
Figure 12-64.  Unfolding details and output files
*CONTROL_FORMING_USER 
Purpose:    This  keyword,  along  with  *CONTROL_FORMING_POSITION,  or  *CON-
TROL_FORMING_TRAVEL, allow user to set up a stamping process simulation.  From 
this card various model parameters may be specified: 
•  material properties, 
•  material model, 
•  tooling kinematics, 
•  mesh adaptivity 
•  D3PLOT generation 
NOTE:  This  option  has  been  deprecated  in  favor  of  *CON-
TROL_FORMING_AUTOPOSITION_PARAME-
TER). 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BLANK 
TYPE 
THICK 
R00 
R45 
R90 
AL/FE 
UNIT 
Type 
I 
Default 
none 
  Card 2 
1 
Variable 
LCSS 
Type 
I 
I 
0 
2 
K 
F 
F 
F 
F 
F 
none 
1.0 
R00 
R00 
3 
N 
F 
4 
E 
F 
5 
6 
DENSITY 
PR 
F 
F 
A 
F 
7 
FS 
F 
I 
1 
8 
MTYPE 
I 
Default 
none 
none 
none 
none 
none 
none 
0.1 
37
Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PATERN 
VMAX 
AMAX 
LVLADA 
SIZEADA  ADATIMS 
D3PLT 
GAP 
Type 
Default 
I 
1 
F 
F 
1000.0  500000.
I 
0 
F 
0 
I 
0 
I 
F 
10 
1.1t 
  VARIABLE   
DESCRIPTION
BLANK 
PID of a sheet blank, as in *PART.  
TYPE 
Flag of part or part set ID for the blank: 
EQ.0: Part ID. 
EQ.1: Part set ID. 
THICK 
R00, R45, 
R90 
AL/FE 
UNIT 
LCSS 
Thickness of the blank.  This variable is ignored if the thickness is
already defined in *SECTION_SHELL. 
Material anisotropic parameters.  For transverse anisotropy the R
value is set to the average value of R00, R45, and R90. 
This  parameter  is  used  to  define  the  Young’s  Modulus,  E,  and
density, ρ, for the sheet blank.  If this variable is defined, E and ρ
will  be  found  by  using  the  proper  unit,  as  listed  in  Table  8.1,
under *CONTROL_FORMING_TEMPLATE. 
EQ.A:  the blank is aluminum  
EQ.F:  the blank is steel (default) 
Units adopted in this simulation.  Define a number between 1 and 
10.  Table 8.1 is used to determine the value for UNIT.  This unit is
used  to  obtain  proper  values  for  punch  velocity,  acceleration,
time step, and physical and material properties. 
If the material for the blank has not been defined, this curve will 
be  used  to  define  the  stress-strain  relation.    Otherwise,  this 
variable is ignored. 
PREBD 
“Pull-over” distance for the upper and lower binders after closing
in a 4-piece stretch draw, as shown in Figure 12-57.
VARIABLE   
DESCRIPTION
K 
N 
E 
Strength coefficient for exponential hardening (𝜎̅̅̅̅̅ = 𝑘𝜀̅ 𝑛).  If LCSS 
is  defined,  or  if  a  blank  material  is  defined  with  *MAT_036  or 
*MAT_037, this variable is ignored. 
Exponent  for  exponential  hardening  (𝜎̅̅̅̅̅ = 𝑘𝜀̅ 𝑛).    If  LCSS  is 
defined,  or  if  a  blank  material  is  defined  with  *MAT_036  or 
*MAT_037, this variable is ignored. 
Young’s Modulus.  If AL/FE is user defined, E is unnecessary. 
DENSITY 
Material density of the blank.  If AL/FE is defined, this variable is 
unnecessary. 
PR 
FS 
MTYP 
Poisson’s  ratio.    If  AL/FE  is  user  defined,  this  variable  is
unnecessary. 
Coulomb  friction  coefficient.    If  contact  is  defined  with  *CON-
TACT_FORMING_..., this variable is ignored. 
Material  model  identification  number,  for  example,  36  for 
*MAT_036 and 37 for *MAT_037.  Currently only material models 
36 and 37 are supported. 
PATERN 
Velocity profile of the moving tool.  If the velocity and the profile
are  defined  by  *BOUNDARY_PRESCRIBED_MOTION_RIGID, 
and *DEFINE_CURVE, this variable is ignored. 
EQ.1: Ramped velocity profile. 
EQ.2: Smooth velocity curve. 
VMAX 
The maximum allowable tool travel velocity. 
AMAX 
The maximum allowable tool acceleration. 
LVLADA 
Maximum mesh adaptive level. 
SIZEADA 
Minimum element size permitted during mesh adaptivity. 
ADATIMS 
Total number of adaptive steps during the simulation. 
D3PLT 
The total number of output states in the D3PLOT database. 
GAP 
Minimum gap between two closing tools at home position, in the
travel direction of the moving tool.  This variable will be used for
*CONTROL_FORMING_POSITION.
Keyword examples: 
A  partial  keyword  example  provided  below  is  for  tools  in  their  home  positions  in  a 
simple 2-piece crash forming die.  A steel sheet blank PID 1, is assigned with a thickness 
of  0.76mm  (UNIT = 1)  and  *MAT_037  with  anisotropic  values  indicated,  to  follow 
hardening  curve  of  90903,  form  in  a  ‘ramped’  type  of  velocity  profile  with  maximum 
velocity  of  5000mm/s  and  acceleration  of  500000.0  mm/s2,  adapt  mesh  5  levels  with 
smallest adapted element size of 0.9 for a total of 20 adaptive steps, create a total of 15 
post-processing  states,  and  to  finish  forming  with  a  final  gap  of  1.1mm  between  the 
tools (PID3 and 5) at home position.  The upper tool with PID 3 is to be moved back in Z 
axis to clear the interference with the blank before close toward the lower tool of target 
PID 5. 
*CONTROL_FORMING_USER 
$    BLANK      TYPE     THICK       R00       R45       R90     AL/FE      UNIT 
         1         0      0.76       1.5       1.6       1.4         F         1 
$     LCSS         K         N         E   DENSITY        PR        FS     MTYPE 
     90903                                                                    37 
$  PATTERN      VMAX      AMAX    LVLADA   SIZEADA   ADATIMS     D3PLT       GAP 
         1    5000.0  500000.0         5       0.9      20.0      15.0       1.1 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*CONTROL_FORMING_POSITION 
$ This is for tools in home position. 
$      PID   PREMOVE    TARGET 
         3                   5 
The following partial keyword example is for tools already positioned in relationship to 
the  blank  and  ready  to  close.    All  assigned  properties  for  the  blank  remain  the  same.  
Here  the  upper  tool  PID3  is  not  going  to  be  moved  back,  but  instead  it  will  move 
forward  to  close  with  the  lower  tool  of  target  PID  5  in  the  direction  specified  by  the 
vector ID 999. 
*CONTROL_FORMING_USER 
         1         0       1.0       1.5       1.6       1.4         F         1 
     90903                                                                    37 
         1    5000.0  500000.0         5       0.9      20.0      15.0       1.1 
*CONTROL_FORMING_TRAVEL 
$      PID       VID    TRAVEL    TARGET       GAP     PHASE    FOLLOW 
         3       999                   5       1.1         1 
Revision information: 
This keyword is available starting in LS-DYNA Revision 48319.
*CONTROL_FREQUENCY_DOMAIN 
Purpose:  Set global control flags and parameters for frequency domain analysis. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
REFGEO 
MPN 
Type 
Default 
I 
0 
F 
0.0 
  VARIABLE   
DESCRIPTION
REFGEO 
Flag for reference geometry in acoustic eigenvalue analysis: 
EQ.0:  use original geometry (t = 0), 
EQ.1:  use deformed geometry at the end of transient analysis.
MPN 
Large mass added per node, to be used in large mass method for
enforced motion. 
Remarks: 
1.  For 
acoustic 
eigenvalue 
keyword 
*FREQUENCY_DOMAIN_ACOUSTIC_  FEM_EIGENVALUE),  sometimes  it  is 
desired to extract the eigenvalues at the end of transient analysis, based on the 
deformed  geometry.    This  is  useful  to  study  the  effect  of  loading  history  on 
acoustic eigenvalues.  In this case, one can set REFGEO = 1 to use the deformed 
geometry at the end of transient analysis. 
analysis 
  in  FRF,  SSD,  or  random  vibration  analysis,  one  can  use  the  large  mass 
method to compute the response.  With the large mass method, the user attach-
es a large mass to the nodes under excitation.  LS-DYNA converts the enforced 
motion  excitation  to  nodal  force  on  the  same  nodes  in  the  same  direction,  to 
produce the desired enforced motion.  MPN is the large mass attached to each 
node under excitation (usually it is in the range of 105-107 times of the original 
mass  of  the  entire  structure).    User  still  need  to  apply  the  large  mass  to  the 
nodes using the keyword *ELEMENT_MASS_{OPTION}. 
The large nodal force p is computed as follows,
For nodal acceleration, 𝑝 = 𝑚𝐿𝑢̈ 
For nodal velocity, 𝑝 = 𝑖 𝜔𝑚𝐿𝑢̇ 
For nodal displacement, 𝑝 = − 𝜔2𝑚𝐿𝑢 
where  𝜔   is  the  round  frequency,  𝑚𝐿  is  the  large  mass  attached  to  each  node 
(MPN), 𝑢̈, 𝑢̇ and 𝑢 are the enforced acceleration, velocity and displacement.
*CONTROL_HOURGLASS_{OPTION} 
Available options include: 
<BLANK> 
936 
The “936” option switches the hourglass formulation for shells so that it is identical to 
that  used  in  LS-DYNA  version  936.    The  modification  in  the  hourglass  control  from 
version  936  was  to  ensure  that  all  components  of  the  hourglass  force  vector  are 
orthogonal  to  rigid  body  rotations.    However,  problems  that  run  under  version  936 
sometimes lead to different results in versions 940 and later.  This difference in results is 
primarily due to the modifications in the hourglass force vector.  Versions released after 
936 should be more accurate. 
Purpose:  Redefine the default values of hourglass control type and coefficient. 
3 
4 
5 
6 
7 
8 
  Card 1 
1 
Variable 
IHQ 
Type 
I 
Default 
2 
QH 
F 
0.1 
Remarks 
1,2 
3,4 
  VARIABLE   
DESCRIPTION
IHQ 
Default hourglass control type: 
EQ.0:  see Remark 1, 
EQ.1:  standard  viscous  form    (may  inhibit  body  rotation  if
solid element shapes are skewed), 
EQ.2:  viscous  form,  Flanagan-Belytschko  integration  for  solid 
elements, 
EQ.3:  viscous  form,  Flanagan-Belytschko  with  exact  volume 
integration for solid elements, 
EQ.4:  stiffness form of type 2 (Flanagan-Belytschko), 
EQ.5:  stiffness  form  of  type  3  (Flanagan-Belytschko)  for  solid
VARIABLE   
DESCRIPTION
elements, 
EQ.6:  Belytschko-Bindeman 
[1993]  assumed 
strain 
co-
rotational stiffness form for 2D and 3D solid elements, 
EQ.7:  Linear total strain form of type 6 hourglass control. 
EQ.8:  Activates  full  projection  warping  stiffness  for  shell
formulations  16  and  -16,  and  is  the  default  for  these 
shell formulations.  A speed penalty of 25% is common
for this option. 
EQ.9:  Puso [2000] enhanced  assumed  strain stiffness form for
3D hexahedral elements, 
EQ.10: Cosserat  Point  Element  (CPE)  developed  by  Jabareen
and  Rubin  [2008]  for  3D  hexahedral  elements  and  Jab-
areen et.al [2013] for 10-noded tetrahedral elements.  See 
Remark 6. 
QH 
Default hourglass coefficient. 
Remarks: 
1.  Hourglass  control  is  viscosity  or  stiffness  that  is  added  to  quadrilateral  shell 
elements  and  hexahedral  solid  elements  that  use  reduced  integration.    It  also 
applies to type 1 tshells.  Without hourglass control, these elements would have 
zero energy deformation modes which could grow large and destroy the solu-
tion.  *CONTROL_HOURGLASS can be used to redefine the default values of 
the hourglass control type and coefficient.  If omitted or if IHQ = 0, the default 
hourglass control types are as follows: 
a)  For shells: viscous type for explicit; stiffness type for implicit.    
b)  For solids: type 2 for explicit; type 6 for implicit. 
c)  For tshell formulation 1:  type 2. 
These  default  values  are  used  unless  HGID  on  *PART  is  used  to  point  to 
*HOURGLASS data which overrides the default values for that part. 
For explicit analysis, shell elements can be used with viscous hourglass control, 
(IHQ = 1 = 2 = 3) or stiffness hourglass control (IHQ = 4 = 5).  Only shell forms 
16 and -16 use the warping stiffness invoked by IHQ = 8.  For implicit analysis, 
the viscous form is unavailable.
For explicit analysis, hexahedral elements can be used with any of the hourglass 
control types except IHQ = 8.  For implicit analysis, only IHQ = 6, 7, 9, and 10 
are available. 
If  IHQ  is  set  to  a  value  that  is  invalid  for  some  elements  in  a  model,  then  the 
hourglass control type for those elements is automatically reset to a valid value.  
For explicit analysis, if IHQ = 6, 7, 9, or 10, then shell elements will be switched 
to type 4 except for form 16 and -16 shells that are switched to type 8.  If IHQ = 
8,  then  solid  elements  and  shell  elements  that  are  not  form  16  or  -16  will  be 
switched to type 4.  For implicit analysis, if IHQ = 1-5, then solid elements will 
be switched to type 6, and if IHQ = 1, 2, 3, 6, 7, 9, or 10, then shell elements will 
switched to type 4. 
2.  Viscous hourglass control has been used successfully with shell elements when 
the response with stiffness based hourglass control was overly stiff.  As models 
have  grown  more  detailed  and  are  better  able  to  capture  deformation  modes, 
there  is  less  need  for  viscous  forms.    To  maintain  back  compatibility,  viscous 
hourglass  control  remains  the  default  for  explicit  analysis,  but  there  may  be 
better choices, particularly the newer forms for bricks (6, 7, 9, and 10). 
3.  QH is a coefficient that scales the hourglass viscosity or stiffness.  With IHQ = 1 
through  5  and  IHQ = 8,  values  of  QH  that  exceed  0.15  may  cause instabilities.  
Hourglass types 6, 7, 9, and 10 will remain stable with larger QH and can work 
well  with  QH =  1.0  for  many  materials.    However,  for  plasticity  models,  a 
smaller value such as QH = 0.1 may work better since the hourglass stiffness is 
based on elastic properties. 
4.  Hourglass  types  6,  7,  9,  and  10  for  hexahedral  elements  are  based  on  physical 
stabilization using an enhanced assumed strain method.  When element meshes 
are not particularly skewed or distorted, their behavior may be very similar and 
all  can  produce  accurate  coarse  mesh  bending  results  for  elastic  material  with 
QH = 1.0.  However, form 9 gives more accurate results for distorted or skewed 
elements.    In  addition,  for  materials  3,  18  and  24  there  is  the  option  to  use  a 
negative value of QH.  With this option, the hourglass stiffness is based on the 
current  material  properties,  i.e.,  the  plastic  tangent  modulus,  and  scaled  by 
|QH|. 
5.  Hourglass  type  7  is  a  variation  on  form  6.    Instead  of  updating  the  hourglass 
forces  incrementally  using  the  current  stiffness  and  an  increment  of  defor-
mations, the total hourglass deformation is evaluated each cycle.  This ensures 
that elements always spring back to their initial geometry if the load is removed 
and the material has not undergone inelastic deformation.  Hourglass type 7 is 
recommended  for  foams  that  employ  *INITIAL_FOAM_REFERENCE_GEOM-
ETRY.  However the CPU time for type 7 is roughly double that for type 6, so it 
is only recommended when needed.
6.  Hourglass type 10 for 1-point solid elements or 10-noded tetrahedron of type 16 
are strucural elements based on Cosserat point theory that allows for accurate 
representation  of  elementary  deformation  modes  (stretching,  bending  and 
torsion) for general element shapes and hyperelastic materials.  To this end, the 
theory in Jabareen and Rubin [2008] and Jabareen et.al [2013] has been general-
ized  in  the  implementation  to  account  for  any  material  response.    The  defor-
mation is separated into a homogenous and an inhomogeneous part where the 
former is treated by the constitutive law and the latter by a hyperelastic formu-
lation that is set up to match analytical results for the deformation modes men-
tioned  above.    Tests  have  shown  that  the  element  is  giving  more  accurate 
results  than  other  hexahedral  elements  for  small  deformation  problems  and 
more realistic behavior in general.
*CONTROL_IMPLICIT 
Purpose:  Set parameters for implicit calculation features. 
*CONTROL_IMPLICIT_AUTO 
*CONTROL_IMPLICIT_BUCKLE 
*CONTROL_IMPLICIT_CONSISTENT_MASS 
*CONTROL_IMPLICIT_DYNAMICS 
*CONTROL_IMPLICIT_EIGENVALUE 
*CONTROL_IMPLICIT_FORMING 
*CONTROL_IMPLICIT_GENERAL 
*CONTROL_IMPLICIT_INERTIA_RELIEF 
*CONTROL_IMPLICIT_JOINTS 
*CONTROL_IMPLICIT_MODAL_DYNAMIC 
*CONTROL_IMPLICIT_MODAL_DYNAMIC_DAMPING_{OPTION} 
*CONTROL_IMPLICIT_MODAL_DYNAMIC_MODE_{OPTION} 
*CONTROL_IMPLICIT_MODES_{OPTION} 
*CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS 
*CONTROL_IMPLICIT_SOLUTION 
*CONTROL_IMPLICIT_SOLVER 
*CONTROL_IMPLICIT_STABILIZATION 
*CONTROL_IMPLICIT_STATIC_CONDENSATION 
*CONTROL_IMPLICIT_TERMINATION
*CONTROL_IMPLICIT_AUTO_{OPTION} 
Available options for OPTION include: 
<BLANK> 
DYN 
SPR 
Purpose:    Define  parameters  for  automatic  time  step  control  during  implicit  analysis 
.  The DYN option allows setting controls 
specifically  for  the  dynamic  relaxation  phase.    The  SPR  option  allows  setting  controls 
specifically for the springback phase. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IAUTO 
ITEOPT 
ITEWIN 
DTMIN 
DTMAX 
DTEXP 
KFAIL 
KCYCLE 
Type 
Default 
I 
0 
I 
11 
I 
5 
F 
F 
F 
DT/1000. DT×10.
none 
  VARIABLE   
DESCRIPTION
IAUTO 
Automatic time step control flag 
EQ.0: constant time step size 
EQ.1: automatically adjust time step size 
EQ.2: automatically adjust time step size and synchronize with
thermal mechanical time step. 
LT.0:  Curve ID = (-IAUTO) gives time step size as a function of 
time.    If  specified,  DTMIN  and  DTMAX  will  still  be  ap-
plied. 
ITEOPT 
ITEWIN 
Optimum  equilibrium  iteration  count  per  time  step.    See  Figure 
12-65. 
Allowable iteration window.  If iteration count is within ITEWIN
iterations  of  ITEOPT,  step  size  will  not  be  adjusted  for  the  next
step.
ITEOPT
+ ITEWIN
ITEOPT
ITEOPT
- ITEWIN
No Auto-Adjust Zone
Figure 12-65.  Iteration Window as defined by ITEOPT and ITEWIN. 
Solution Time
  VARIABLE   
DTMIN 
DESCRIPTION
Minimum  allowable  time  step  size.    Simulation  stops  with  error
termination if time step falls below DTMIN. 
DTMAX 
Maximum allowable time step size. 
DTEXP 
KFAIL 
LT.0:  curve ID = (-DTMAX) gives max step size as a function of 
time.  Also, the step size is adjusted automatically so that 
the time value of each point in the curve is reached exact-
ly . 
Time interval to run in explicit mode before returning to implicit
mode.  Applies only when automatic implicit-explicit switching is 
active  (IMFLAG = 4  or  5  on  *CONTROL_IMPLICIT_GENERAL). 
Also, see KCYCLE. 
EQ.0: defaults to the current implicit time step size. 
LT.0:  curve ID = (-DTEXP) gives the time interval as a function 
of time. 
Number  of  failed  attempts  to  converge  implicitly  for  the  current
time  step  before  automatically  switching  to  explicit  time
integration. 
  Applies  only  when  automatic  implicit-explicit 
switching is active.  The default is one attempt.  If IAUTO = 0, any 
input value is reset to unity.
DT0
DTMAX > 0
DTMAX > 0
time step value
DTMIN
DTMIN
Time
Figure 12-66.  The implicit time step size changes continuously as a function
of convergence within the bounds set by DTMIN and DTMAX 
  VARIABLE   
KCYCLE 
Remarks: 
  VARIABLE   
IAUTO 
ITEOPT 
DESCRIPTION
Number of explicit cycles to run in explicit mode before returning
to the implicit mode.  The actual time interval that is used will be 
the  maximum  between  DTEXP  and  KCYCLE*(latest  estimate  of
the explicit time step size). 
REMARK
The  default  for  IAUTO  depends  on  the  analysis  type.    For
“springback”  analysis,  automatic  time  step  control  and  artificial
stabilization are activated by default. 
With IAUTO = 1 or 2, the time step size is adjusted if convergence
is reached in a number of iterations that falls outside the specified
“iteration window”, increasing after “easy” steps, and decreasing
  ITEOPT  defines  the
after  “difficult”  but  successful  steps. 
midpoint  of  the  iteration  window.    A  value  of  ITEOPT = 30  or 
more  can  be  more  efficient  for  highly  nonlinear  simulations  by 
allowing more iterations in each step, hence fewer total steps. 
ITEWIN 
The  step  size  is  not  adjusted  if  the  iteration  count  falls  within
ITEWIN of ITEOPT.  Large values of ITEWIN make the controller
more tolerant of variations in iteration count.
2.0
1.0
0.0
-1.0
DTMAX active from previous key point
to current key point
A key point is automatically
generated at the termination time
Problem Time
end
negative value ⇒ d3plot output
suppressed
= Load curve points (DTMAX < 0), also key points
= LS-DYNA generated key point
Figure 12-67.  DTMAX < 0.  The maximum time step is set by a load curve of
LCID = −DTMAX interpolated using piecewise constants.  The abscissa values
of  the  load  curve  determine  the  set  of  key  points.    The  absolute  value  of  the
ordinate  values  set  the  maximum  time  step  size.    Key  points  are  special  time
values for which the  integrator will  adjust the time step so as to  reach exactly.
For each key point with a positive function value, LS-DYNA will write the state
to the binary database. 
  VARIABLE   
DTMAX 
DTEXP 
REMARK
To  strike  a  particular  simulation  time  exactly,  create  a  key  point
curve  (Figure  12-67)  and  enter  DTMAX = -(curve  ID).    This  is 
useful  to  guarantee  that  important  simulation  times,  such  as
when peak load values occur, are reached exactly. 
When the automatic implicit-explicit switching option is activated 
(IMFLAG = 4  or  5  on  *CONTROL_IMPLICIT_GENERAL),  the 
solution method will begin as implicit, and if convergence of the
equilibrium  iterations  fails,  automatically  switch  to  explicit  for  a
time  interval  of  DTEXP.    A  small  value  of  DTEXP  should  be 
chosen so that significant dynamic effects do not develop during 
the  explicit  phase,  since  these  can  make  recovery  of  nonlinear
equilibrium  difficult  during  the  next  implicit  time  step.    A
reasonable  starting  value  of  DTEXP  may  equal  several  hundred
VARIABLE   
REMARK
explicit time steps.
*CONTROL_IMPLICIT_BUCKLE 
Purpose:  Activate implicit buckling analysis when termination time is reached .    Optionally,  buckling  analyses  are    performed  at 
intermittent times. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NMODE  BCKMTH 
Type 
I 
I 
Default 
0 
see 
below 
  VARIABLE   
DESCRIPTION
NMODE 
Number of buckling modes to compute 
EQ.0:  none (DEFAULT) 
GT.0:  compute n lowest buckling modes 
LT.0:  curve  ID = (-NEIG)  used  for 
intermittent  buckling 
analysis 
BCKMTH 
Method used to extract buckling modes  
EQ.1: Use  Block  Shift  and  Invert  Lanczos.    Default  of  all
problems  not  using  *CONTROL_IMPLICIT_INERTIA_-
RELIEF. 
EQ.2: Use  Power  Method.    Only  valid  option  for  problems
using  *CONTROL_IMPLICIT_INERTIA_RELIEF.    Op-
tional for other problems.  See Remarks. 
Remarks: 
Buckling analysis is performed at the end of a static implicit simulation or at specified 
times  during  the  simulation.    The  simulation  may  be  linear  or  nonlinear  but  must  be 
implicit.    After  loads  have  been  applied  to  the  model,  the  buckling  eigenproblem  is 
solved: 
[𝐊𝑀 + 𝜆𝐊𝐺]{𝑢} = 0
where  𝐊𝑀  is  the  material  tangent  stiffness  matrix,  and  the  geometric  or  initial  stress 
stiffness  matrix  𝐊𝐺  is  a  function  of  internal  stress  in  the  model.    The  lowest  n 
eigenvalues  and  eigenvectors  are  computed.    The  eigenvalues,  written  to  text  file 
“eigout”,  represent  multipliers  to  the  applied  loads  which  give  buckling  loads.    The 
eigenvectors,  written  to  binary  database  “d3eigv”,  represent  buckling  mode  shapes.  
View and animate these modes using LS-PrePost.  When NMODE > 0, eigenvalues will 
be computed at the termination time and LS-DYNA will terminate. 
When  NMODE < 0,  an  intermittent  buckling  analysis  will  be  performed.    This  is  a 
transient  simulation  during  which  loads  are  applied,  with  buckling  modes  computed 
periodically during the simulation.  Changes in geometry, stress, material, and contact 
conditions  will  affect  the  buckling  modes.    The  transient  simulation  must  be  implicit.  
The curve ID = -NMODE indicates when to extract the buckling modes, and how many 
to extract.  Define one curve point at each desired extraction time, with a function value 
equal to the number of buckling modes desired at that time.  A d3plot database will be 
produced for the transient solution results.  Consecutively numbered d3eigv and eigout 
databases  will  be  produced  for  each  intermittent  extraction.    The  extraction  time  is 
indicated in each database’s analysis title. 
The buckling modes can be computed using either Block Shift and Invert Lanczos or the 
Power  Method.    It  is  strongly  recommended  that  the  Block  Shift  and  Invert  Lanczos 
method  is  used  as  it  is  a  more  powerful  and  robust  algorithm.    For  problems  using 
*CONTROL_IMPLICIT_INERTIA_RELIEF  the  Power  Method  must  be  used  and  any 
input value for BCKMTH will be overridden with the required value of 2.  There may 
be  some  problems,  which  are  not  using  *CONTROL_IMPLICIT_INERTIA_RELIEF, 
where  the  Power  Method  may  be  more  efficient  than  Block  Shift  and  Invert  Lanczos.  
But  the  Power  Method  is  not  as  robust  and  reliable  as  Lanczos  and  results  should  be 
verified.    Furthermore  convergence  of  the  Power  Method  is  better  for  buckling 
problems  where  the  expected  buckling  mode  is  close  to  one  in  magnitude  and  the 
dominant  mode  is  separated  from  the  secondary  modes.    The  number  of  modes 
extracted via the Power Method should be kept in the range of 1 to 5. 
The  geometric  stiffness  terms  needed  for  buckling  analysis  will  be  automatically 
computed  when  the  buckling  analysis  time  is  reached,  regardless  of  the  value  of  the 
geometric stiffness flag IGS on *CONTROL_IMPLICIT_GENERAL. 
A double precision executable should be used for best accuracy in buckling analysis. 
Parameters  CENTER,  LFLAG,  LFTEND,  RFLAG,  RHTEND  and  SHFSCL  from  *CON-
TROL_IMPLICIT_EIGENVALUE  are  applicable  to  buckling  analysis.    For  buckling 
analysis  CENTER,  LFTEND,  RHTEND  and  SHFSCL  are  in  units  of  the  eigenvalue 
spectrum.
*CONTROL_IMPLICIT_CONSISTENT_MASS 
Purpose:  Use the consistent mass matrix in implicit dynamics and eigenvalue solutions. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IFLAG 
Type 
Default 
I 
0 
  VARIABLE   
DESCRIPTION
IFLAG 
Consistent mass matrix flag 
EQ.0: Use the standard lumped mass formulation (DEFAULT)
EQ.1: Use the consistent mass matrix. 
Remarks: 
The  consistent  mass  matrix  formulation  is  currently  available  for  the  three  and  four 
node shell elements, solid elements types 1, 2, 10, 15, 16, and 18 , and beam types 1, 2, 3, 4, and 5 .   All other element types 
continue to use a lumped mass matrix.
*CONTROL_IMPLICIT_DYNAMICS_{OPTION} 
Available options include: 
<BLANK> 
DYN 
SPR 
Purpose:  Activate implicit dynamic analysis and define time integration constants .    The  DYN  option  allows  setting  controls 
specifically  for  the  dynamic  relaxation  phase.    The  SPR  option  allows  setting  control 
specifically for the springback phase. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IMASS 
GAMMA 
BETA 
TDYBIR 
TDYDTH 
TDYBUR 
IRATE 
ALPHA 
Type 
Default 
I 
0 
F 
F 
F 
F 
F 
.50 
.25 
0.0 
1028 
1028 
I 
0 
F 
0 
  VARIABLE   
DESCRIPTION
IMASS 
Implicit analysis type 
LT.0:  curve  ID = (-SCALE)  used  to  control  amount  of  implicit 
  TDYBIR,
dynamic  effects  applied  to  the  analysis. 
TDYDTH and TDYBUR are ignored with this option. 
EQ.0: static analysis 
EQ.1: dynamic analysis using Newmark time integration. 
EQ.2: dynamic  analysis  by  modal  superposition  following  the 
solution of the eigenvalue problem 
EQ.3: dynamic  analysis  by  modal  superposition  using  the
eigenvalue  solution  in  the  d3eigv  files  that  are  in  the 
runtime directory. 
GAMMA 
Newmark time integration constant . 
BETA 
Newmark time integration constant .
100%
0%
TDYBIR
TDYDTH
TDYBUR
Time
Figure  12-68.    Birth,  death,  and  burial  time  for  implicit  dynamics.    The  terms
involving  𝑴  and  𝑫  are  scaled  by  a  factor  between  ranging  between  1  and  0  to
include or exclude dynamical effects, respectively. 
  VARIABLE   
DESCRIPTION
TDYBIR 
Birth time for application of dynamic terms.   See Figure 12-68. 
TDYDTH 
Death time for application of dynamic terms. 
TDYBUR 
Burial time for application of dynamic terms. 
IRATE 
Rate effects switch: 
EQ.0: rate effects are on in constitutive models 
EQ.1: rate effects are off in constitutive models 
EQ.2: rate effects are off in constitutive models for both explicit 
and implicit. 
ALPHA 
Composite time integration constant . 
GT.0:  Bathe composite scheme is activated 
LT.0:  HHT scheme is activated 
Remarks: 
For  the  dynamic  problem,  the  linearized  equilibrium  equations  may  be  written  in  the 
form
𝑴𝒖̈𝑛+1 + 𝑫𝒖̇𝑛+1 + 𝑲𝑡(𝒙𝑛)Δ𝒖 = 𝑷(𝒙𝑛)𝑛+1 − 𝑭(𝒙𝑛) 
where 
𝑴 = lumped mass matrix 
𝑫 = damping matrix 
𝒖𝑛+1 = 𝒙𝑛+1 − 𝒙0 = nodal displacement vector 
𝒖̇𝑛+1 = nodal point velocities at time 𝑛 + 1 
𝒖̈𝑛+1 = nodal point acceleration at time 𝑛 + 1 
Between  the  birth  and  death  times  100%  of  the  dynamic  terms,  that  is  the  terms 
involving M and D, are applied.  Between the death and burial time the dynamic terms 
are  decreased  linearly  with  respect  to  time  until  0%  of  the  dynamic  terms  are  applied 
after  the  burial  time.    This  feature  is  useful  for  problems  that  are  initially  singular 
because  the  parts  are  not  in  contact  initially  such  as  in  metal  stamping.    For  these 
problems dynamics is required for stable convergence.  When contact is established the 
problem  becomes  well  conditioned  and  the  dynamic  terms  are  no  longer  required  for 
stable convergence.  It is recommend that for such problems the user set the death time 
to be after contact is established and the burial time for 2 or 3 time steps after the death 
time. 
For problems with more extensive loading and unloading patterns the user can control 
the  amount  of  dynamic  effects  added  to  the  model  by  using  a  load  curve,  see 
IMASS.LT.0.    This  curve  should  have  ordinate  values  between  0.0  and  1.0.    The  user 
should use caution in ramping the load curve and the associated dynamic effects from 
1.0 to 0.0.  Such a ramping down should take place over 2 or 3 implicit time steps. 
The time integration is by default the unconditionally stable, one-step, Newmark-β time 
integration scheme 
𝒖̈𝑛+1  =
Δ𝒖
𝛽Δ𝑡2 −
𝒖̇𝑛
𝛽Δ𝑡
−
(
− 𝛽) 𝒖̈𝑛 
𝒖̇𝑛+1 = 𝒖̇𝑛 + Δ𝑡(1 − 𝛾)𝒖̈𝑛 + 𝛾Δ𝑡𝒖̈𝑛+1 
𝒙𝑛+1 = 𝒙𝑛 + Δ𝒖 
Here, Δ𝑡  is  the  time  step  size,  and  𝛽  and 𝛾  are the  free  parameters of  integration.   For 
𝛾 = 1
4⁄   the  method  reduces  to  the  trapezoidal  rule  and  is  energy 
2⁄   and  𝛽 = 1
conserving.  If 
γ >
𝛽 >
+ 𝛾)
 , 
(
Then  numerical  damping  is  induced  into  the  solution  leading  to  a  loss  of  energy  and 
momentum. 
The  Newmark  method,  and  the  trapezoidal  rule  in  particular,  is  known  to  lack  the 
robustness required for simulating long term dynamic implicit problems.  Even though 
numerical  damping  may improve the situation from this aspect, it is difficult to know 
how to set 𝛾 and 𝛽 without deviating from desired physical properties of the system.  In 
the  literature,  a  vast  number  of  composite  time  integration  algorithms  have  been 
proposed to handle this, and a family of such methods is implemented and governed by 
the  value  of  𝛼  (ALPHA,  parameter  8  on  card  1).    For  𝛼 > 0,  every  other  implicit  time 
step is a three point backward Euler step given as 
𝒖̈𝑛+1  =
(1 + 𝛼)
∆𝑡
(𝒖̇𝑛+1 − 𝒖̇𝑛) −
∆𝑡−
(𝒖̇𝑛 − 𝒖̇𝑛−1) 
Δ𝒖 −
Δ𝒖− 
𝒖̇𝑛+1 =
(1 + 𝛼)
∆𝑡
∆𝑡−
where ∆𝑡− = 𝑡𝑛 − 𝑡𝑛−1  and  Δ𝒖− = 𝒖𝑛 − 𝒖𝑛−1  are  constants.    Because  of  this  three  step 
procedure,  the  method  is  particularly  suitable  for  nodes/bodies  undergoing  curved 
motion as it better accounts for curvature than the default Newmark step.  For 𝛼 = 1/2, 
and  default  values  of  𝛾  and  𝛽,  the  method  defaults  to  the  Bathe  time  integration 
scheme,  Bathe  [2007],  and  is  reported  to  preserve  energy  and  momentum  to  a 
reasonable  degree.    The  improvement  in  stability  over  the  Newmark  method  is 
primarily attributed to numerical dissipation, but fortunately this dissipation appears to 
mainly  be  due  to  damping  of  high  frequency  content  and  the  underlying  physics  is 
therefore not affected as such, see Bathe and Nooh [2012]. 
For  a  negative  value  of  ALPHA,  the  HHT,  Hilber-Hughes-Taylor  [1977],  scheme  is 
activated.  This scheme is similar to that of the Newmark method, but the equilibrium is 
sought  at  time  step  𝑛 + 1 + 𝛼  instead  of  at  𝑛 + 1.    As  a  complement  to  the  Newmark 
scheme above, we introduce 
𝒖̇𝛼 = −𝛼𝒖̇𝑛 + (1 + 𝛼)𝒖̇𝑛+1 
𝒙𝛼 = −𝛼𝒙𝑛 + (1 + 𝛼)𝒙𝑛+1 
and solve a modified system of equilibrium equations 
𝑴𝒖̈𝑛+1 + 𝑫𝒖̇𝛼 + 𝑭(𝒙𝛼) = 𝑷(𝒙𝛼). 
3 ≤ 𝛼 ≤ 0  and  𝛾 = 1−2𝛼
This  method  is  stable  for  − 1
,  which  becomes  the 
default  values  of  𝛾  and  𝛽  if  not  explicitly  set.    Parameter  𝛼  controls  the  amount  of 
dissipation  in  the  problem,  for  𝛼 = 0  an  undamped  Newmark  scheme  is  obtained, 
whereas  𝛼 = − 1
3  introduces  significant  damping.    From  the  literature,  a  value  of 
𝛼 = −0.05 appears to be a good choice. 
2   and  𝛽 = (1−𝛼)2
When modal superposition is invoked, NEIGV on *CONTROL_IMPLICIT_EIGENVAL-
UE indicates the number of modes to be used.  With modal superposition, stresses are 
computed only for linear shell formulation 18.
*CONTROL_IMPLICIT_EIGENVALUE 
Purpose:  Activate implicit eigenvalue analysis and define associated input parameters 
. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NEIG 
CENTER 
LFLAG 
LFTEND 
RFLAG 
RHTEND 
EIGMTH 
SHFSCL 
Type 
Default 
I 
0 
This card is optional. 
F 
I 
F 
I 
F 
I 
F 
0.0 
0 
-infinity
0 
+infinity 
2 
0.0 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ISOLID 
IBEAM 
ISHELL 
ITSHELL  MSTRES  EVDUMP  MSTRSCL 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
F 
0.001 
  VARIABLE   
NEIG 
DESCRIPTION
Number  of  eigenvalues  to  extract.    This  must  be  specified.    The
other parameters below are optional. 
LT.0:  curve  ID = (-NEIG)  used  for  intermittent  eigenvalue 
analysis 
CENTER 
  This  option 
Center 
eigenvalues located about this value. 
frequency. 
finds 
the  nearest  NEIG
LFLAG 
Left end point finite flag. 
EQ.0: left end point is -infinity 
EQ.1: left end point is LFTEND. 
LFTEND 
Left end point of interval.  Only used when LFLAG = 1.
VARIABLE   
DESCRIPTION
RFLAG 
Right end point finite flag: 
EQ.0: right end point is +infinity 
EQ.1: right end point is RHTEND. 
RHTEND 
Right end point of interval.  Only used when RFLAG = 1. 
EIGMTH 
Eigenvalue extraction method: 
EQ.2: Block Shift and Invert Lanczos (default). 
EQ.3: Lanczos with [M] = [I] (for debug only). 
EQ.5: Same as 3 but include Dynamic Terms 
SHFSCL 
Shift scale.  Generally not used, but see explanation below. 
ISOLID 
IBEAM 
ISHELL 
ITSHELL 
If nonzero, reset all solid element formulations to ISOLID for the
implicit computations.  Can be used for all implicit computations
not just eigenvalue computations. 
If nonzero, reset all beam element formulations to IBEAM for the
implicit computations.  Can be used for all implicit computations
not just eigenvalue computations. 
If nonzero, reset all shell element formulations to ISHELL for the
implicit computations.  Can be used for all implicit computations
not just eigenvalue computations. 
If nonzero, reset all thick shell element formulations to ITSHELL
for  the  implicit  computations.    Can  be  used  for  all  implicit
computations not just eigenvalue computations. 
MSTRES 
Flag for computing the stresses for the eigenmodes: 
EQ.0: Do not compute the stresses. 
EQ.1: Compute the stresses.
EVDUMP 
*CONTROL_IMPLICIT_EIGENVALUE 
DESCRIPTION
Flag  for  writing  eigenvalues  and  eigenvectors  to  file  “Eigen_
Vectors” (SMP only): 
EQ.0: Do not write eigenvalues and eigenvectors. 
GT.0: Write  eigenvalues  and  eigenvectors  using  an  ASCII
format. 
LT.0:  Write  eigenvalues  and  eigenvectors  using  a  binary
format. 
MSTRSCL 
Scaling  for  computing  the  velocity  based  on  the  mode  shape  for
the stress computation. 
Remarks: 
To  perform  an  eigenvalue  analysis,  activate  the  implicit  method  by  selecting  IM-
FLAG = 1  on  *CONTROL_IMPLICIT_GENERAL,  and  indicate  a  nonzero  value  for 
NEIG  above.    By  default,  the  lowest  NEIG  eigenvalues  will  be  found.    If  a  nonzero 
center frequency is specified, the NEIG eigenvalues nearest to CENTER will be found. 
When  NEIG > 0,  eigenvalues  will  be  computed  at  time = 0  and  LS-DYNA  will 
terminate. 
When  NEIG < 0,  an  intermittent  eigenvalue  analysis  will  be  performed.    This  is  a 
transient  simulation  during  which  loads  are  applied,  with  eigenvalues  computed 
periodically during the simulation.  Changes in geometry, stress, material, and contact 
conditions will affect the eigenvalues.  The transient simulation can be either implicit or 
explicit  according  to  IMFLAG = 1  or  IMFLAG = 6,  respectively,  on  *CONTROL_IM-
PLICIT_GENERAL.  The curve ID = -NEIG indicates when to extract eigenvalues, and 
how  many  to  extract.    Define  one  curve  point  at  each  desired  extraction  time,  with  a 
function  value  equal  to  the  number  of  eigenvalues  desired  at  that  time.    A  d3plot 
database will  be produced for the transient solution results.  Consecutively numbered 
d3eigv  and  eigout  databases  will  be  produced  for  each  intermittent  extraction.    The 
extraction time is indicated in each database’s analysis title. 
The  Block  Shift  and  Invert  Lanczos  code  is  from  BCSLIB-EXT,  Boeing's  Extreme 
Mathematical Library.  
When  using  Block  Shift  and  Invert  Lanczos,  the  user  can  specify  a  semifinite  or  finite 
interval  region  in  which  to  compute  eigenvalues.    Setting  LFLAG = 1  changes  the  left 
end point from -infinity to the value specified by LFTEND.  Setting RFLAG = 1 changes 
the  right  end  point  from  +infinity  to  the  values  given  by  RHTEND.    If  the  interval 
includes  CENTER  (default  value  of  0.0)  then  the  problem  is  to  compute  the  NEIG
eigenvalues nearest to CENTER.  If the interval does not include CENTER, the problem 
is to compute the smallest in magnitude NEIG eigenvalues. 
If all of the eigenvalues are desired in an interval where both end points are finite just 
input a large number for NEIG.  The software will automatically compute the number 
of eigenvalues in the interval and lower NEIG to that value.  The most general problem 
specification  is  to  compute  NEIG  eigenvalues  nearest  CENTER  in  the  interval 
[LFTEND,RHTEND].    Computing  the  lowest  NEIG  eigenvalues  is  equivalent  to 
computing the NEIG eigenvalues nearest 0.0. 
For  some  problems  it  is  useful  to  override  the  internal  heuristic  for  picking  a  starting 
point for Lanczos shift strategy, that is the initial shift.  In these rare cases, the user may 
specify the initial shift via the parameter SHFSCL.  SHFSCL should be in the range of 
first few nonzero frequencies. 
Parameters  CENTER,  LFTEND,  RHTEND,  and  SHFSCL  are  in  units  of  Hertz  for 
eigenvalue  problems.    These  four  parameters  along  with  LFLAG  and  RFLAG  are 
applicable  for  buckling  problems..    For  buckling  problems  CENTER,  LFTEND, 
RHTEND, and SHFSCL are in units of the eigenvalue spectrum. 
Eigenvectors are written to an auxiliary binary plot database named “d3eigv”, which is 
automatically created.  These can be viewed using a postprocessor in the same way as a 
standard "d3plot" database.  The time value associated with each eigenvector plot is the 
corresponding  frequency  in  units  of  cycles  per  unit  time.    A  summary  table  of 
eigenvalue results is printed to the "eigout" file.  In addition to the eigenvalue results, 
modal participation factors and modal effective mass tables are written to the “eigout” 
file.  The user can export individual eigenvectors using LSPrePost.  
The  user  can  request  stresses  to  be  computed  and  written  to  d3eigv  via  MSTRES.    A 
velocity is computed by dividing the displacements from the eigenmode by MSTRSCL.  
The  element  routine  then  computes  the  stresses  based  on  this  velocity,  but  then  those 
stresses  are  inversely  scaled  by  MSTRSCL  before  being  written  to  d3eigv.    Thus 
MSTRSCL  has  no  effect  on  results  of  linear  element  formulations.    The  strains 
associated with the stresses output using the MSTRES option can be obtained by setting 
the STRFLG on *DATABASE_EXTENT_BINARY. 
Eigenvalues and eigenvectors can be written to file “Eigen_Vectors” by using a nonzero 
value for EVDUMP.  If EVDUMP > 0 an ASCII file is used.  If EVDUMP < 0 a simple 
binary  format  is  used.    The  binary  format  is  to  reduce  file  space.    The  eigenvectors 
written  to  this  file  will  be  orthonormal  with  respect  to  the  mass  matrix.    Eigenvector 
dumping is an SMP only feature. 
The  print  control  parameter,  LPRINT,  and  ordering  method  parameter,  ORDER,  from 
the  *CONTROL_IMPLICIT_SOLVER  keyword  card  also  apply  to  the  Block  Shift  and 
Invert Eigensolver.
*CONTROL_IMPLICIT_FORMING_{OPTION} 
Available options include: 
<BLANK> 
DYN 
SPR 
Purpose:  This keyword is used to perform implicit static analysis, especially for metal 
forming  processes,  such  as  gravity  loading,  binder  closing,  flanging,  and  stamping 
subassembly  simulation.    A  systematic  study  had  been  conducted  to  identify  the  key 
factors  affecting  implicit  convergence,  and  the  preferred  values  are  automatically  set 
with this keyword.  In addition to forming application, this keyword can also be used in 
other applications, such as dummy loading and roof crush, etc.  The DYN option allows 
setting  controls  specifically  for  the  dynamic  relaxation  phase.    The  SPR  option  allows 
setting controls specifically for the springback phase. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IOPTION 
NSMIN 
NSMAX 
BIRTH 
DEATH 
PENCHK 
Type 
Default 
I 
1 
I 
none 
I 
2 
F 
F 
F 
0.0 
1.e+20 
0.0 
  VARIABLE   
DESCRIPTION
IOPTION 
Solution type: 
EQ.1: Gravity loading simulation, see remarks below. 
EQ.2: Binder  closing  and  flanging  simulation,  see  remarks
below. 
NSMIN 
Minimum number of implicit steps for IOPTION = 2. 
NSMAX 
Maximum number of implicit steps for IOPTION = 2. 
BIRTH 
Birth time to activate this feature. 
DEATH 
Death time.
DESCRIPTION
Relative allowed penetration with respect to the part thickness in
contact for IOPTION = 2.   
time 
Initial 
in
*CONTROL_IMPLICIT_GENERAL, which is no longer needed if
DT0 is specified here. 
defined 
size, 
step 
as 
  VARIABLE   
PENCHK 
DT0 
General remarks: 
This  keyword  provides  a  simplified  interface  for  implicit  static  analysis.    If  no  other 
implicit  cards  are  used,  the  stiffness  matrix  is  reformed  every  iteration.    Convergence 
tolerances  (DCTOL,  ECTOL,  etc.)  are  automatically  set  and  recommended  no  to  be 
changed.  In almost all cases, only two additional implicit control cards (*CONTROL_-
IMPLICIT_GENERAL, and_AUTO) may be needed to control the stepping size, where 
variables DT0, DTMIN and DTMAX can be used for control.  
If  multiple  steps  are  required  for  IOPTION = 1,  *CONTROL_IMPLICIT_GENERAL 
must be placed after *CONTROL_IMPLICIT_FORMING with DT0 specified as a certain 
fraction of the ENDTIM .  Otherwise, even with DT0 
specified as a fraction of the ENDTIM, only one step (with step size of ENDTIM) will be 
performed. 
As  always,  the  variable  IGAP  should  be  set  to  “2”  in  *CONTACT_FORMING…  cards 
for  a  more  realistic  contact  simulation  in  forming.    The  contact  type  *CONTACT_-
FORMING_SURFACE_TO_SURFACE  is  recommended  to  be  used  with  implicit 
analysis. 
Smaller  penalty  stiffness  scale  factor  SLSFAC  produces  a  certain  amount  of  contact 
penetration but yields faster simulation time, and therefore is recommended for gravity 
and  closing  (in  case  of  no  physical  beads)  simulation.    Subsequent  forming  process  is 
likely  to  follow  and  contact  conditions  will  be  reestablished  there,  where  a  tighter, 
default SLSFAC (0.1) should be used. 
It is recommended that the fully integrated element type 16 is to be used for all implicit 
calculation.  For solids, type “-2” is recommended.   
Executable with double precision is to be used for all implicit calculation. 
Models with over 100,000 deformable elements are more efficient to be simulated with 
MPP for faster turnaround time.
*CONTROL_IMPLICIT_FORMING 
An  example  of  the  implicit  gravity  is  provided  below,  where  a  blank  is  loaded  with 
gravity into a toggle die.  A total of five steps are used, controlled by the variable DT0.  
The  results  are  shown  in  Figure  12-69.    If  this  binder  closing  is  done  with  explicit 
dynamics, efforts need to be made to reduce the inertia effects on the blank since contact 
with the upper binder only happens along the periphery and a large middle portion of 
the blank is not driven or supported by anything.  With implicit static method, there is 
no inertia effect at all on the blank during the closing, and no tool speed, time step size, 
etc.  to be concerned about. 
The  implicit  gravity  application  for  both  air  and  toggle  draw  process  is  available 
through  LS-PrePost  4.0  in  Metal  Forming  Application/eZ  Setup  (http://ftp.lstc.com/-
anonymous/outgoing/lsprepost/4.0/metalforming/). 
*KEYWORD 
*PARAMETER 
⋮  
*CONTROL_TERMINATION 
1.0 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*CONTROL_IMPLICIT_FORMING 
$  IOPTION 
         1 
*CONTROL_IMPLICIT_GENERAL 
$   IMFLAG       DT0 
         1       0.2 
*CONTROL_CONTACT 
$   SLSFAC    RWPNAL    ISLCHK    SHLTHK    PENOPT    THKCHG     ORIEN 
      0.03       0.0         2         1         4         0         4 
$   USRSTR    USRFAC     NSBCS    INTERM     XPENE     SSTHK      ECDT   TIEDPRJ 
         0         0        10         0       1.0         0 
*PART 
 Blank 
   &blkpid   &blksec   &blkmid                                 
*SECTION_SHELL 
$      SID    ELFORM      SHRF       NIP     PROPT   QR/IRID     ICOMP     SETYP 
&blksec           16     0.833         7       1.0 
$       T1        T2        T3        T4      NLOC 
&bthick,&bthick,&bthick,&bthick 
*CONTACT_FORMING_SURFACE_TO_SURFACE 
$     SSID      MSID     SSTYP     MSTYP    SBOXID    MBOXID       SPR       MPR 
   &blksid  &lpunsid         2         2                             1         1 
$       FS        FD        DC        VC       VDC    PENCHK        BT        DT 
      0.12       0.0       0.0       0.0      20.0         0       0.0     1E+20 
$      SFS       SFM       SST       MST      SFST      SFMT       FSF       VSF 
       1.0       1.0       0.0     &mstp 
$     SOFT    SOFSCL    LCIDAB    MAXPAR    PENTOL     DEPTH     BSORT    FRCFRQ 
         0 
$   PENMAX    THKOPT    SHLTHK     SNLOG      ISYM     I2D3D    SLDTHK    SLDSTF 
                                       1 
$     IGAP    IGNORE    DPRFAC    DTSTIF                        FLANGL 
         2 
⋮  
*LOAD_BODY_Z 
90994 
*DEFINE_CURVE_TITLE 
Body Force on blank 
90994
0.0,9810.0 
10.0,9810.0 
*LOAD_BODY_PARTS 
&blksid 
*END 
Binder closing example: 
An  example  of  binder  closing  and  its  progression  is  shown  in  Figures  12-70,  12-71, 
12-72,  and  12-73,  using  the  NUMISHEET’05  deck  lid  inner,  where  a  blank  is  being 
closed  in  a  toggle  die  (modified).    An  adaptive  level  of  three  was  used  in  the  closing 
process.  Gravity is and should be always applied at the same time, regardless if a prior 
gravity  loading  simulation  is  performed  or  not,  as  listed  at  the  end  of  the  input  deck.  
The  presence  of  the  gravity  helps  the  blank  establish  an  initial  contact  with  the  tool, 
thus  improving  the  convergence  rate.    The  upper  binder  is  moved  down  by  a  closing 
distance (defined  by a parameter &bindmv) using a displacement  boundary condition 
(VAD = 2),  with  a  simple  linearly  increased  triangle-shaped  load  curve.    The  variable 
DT0  is  set  at  0.01,  determined  by  the  expected  total  deformation.    The  solver  will 
automatically adjust based on the initial contact condition.  The maximum  step size  is 
controlled by the variable DTMAX, and this value needs to be sufficiently small (<0.02) 
to  avoid  missing  contact,  but  yet  not  too  small  causing  a  long  running  time.    In  some 
cases, this variable can be set larger, but the current value works for most cases. 
*KEYWORD 
*PARAMETER 
⋮  
*CONTROL_TERMINATION 
1.0 
*CONTROL_IMPLICIT_FORMING 
$  IOPTION     NSMIN     NSMAX 
         2         2       100 
*CONTROL_IMPLICIT_GENERAL 
$   IMFLAG       DT0 
         1      0.01 
*CONTROL_IMPLICIT_AUTO 
$    IAUTO    ITEOPT    ITEWIN     DTMIN     DTMAX 
         0         0         0      0.01      0.03 
*CONTROL_ADAPTIVE 
⋮  
*CONTROL_CONTACT 
$   SLSFAC    RWPNAL    ISLCHK    SHLTHK    PENOPT    THKCHG     ORIEN 
      0.03       0.0         2         1         4         0         4 
$   USRSTR    USRFAC     NSBCS    INTERM     XPENE     SSTHK      ECDT   TIEDPRJ 
         0         0        10         0       1.0         0 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
⋮  
*PART 
 Blank 
$      PID     SECID       MID     EOSID      HGID      GRAV    ADPOPT      TMID 
   &blkpid   &blksec   &blkmid                                 &adpyes 
*SECTION_SHELL 
$      SID    ELFORM      SHRF       NIP     PROPT   QR/IRID     ICOMP     SETYP 
&blksec           16     0.833         7       1.0 
$       T1        T2        T3        T4      NLOC 
&bthick,&bthick,&bthick,&bthick 
⋮  
*CONTACT_FORMING_SURFACE_TO_SURFACE
$     SSID      MSID     SSTYP     MSTYP    SBOXID    MBOXID       SPR       MPR 
   &blksid  &lpunsid         2         2                             1         1 
$       FS        FD        DC        VC       VDC    PENCHK        BT        DT 
      0.12       0.0       0.0       0.0      20.0         0       0.0     1E+20 
$      SFS       SFM       SST       MST      SFST      SFMT       FSF       VSF 
       1.0       1.0       0.0     &mstp 
$     SOFT    SOFSCL    LCIDAB    MAXPAR    PENTOL     DEPTH     BSORT    FRCFRQ 
         0 
$   PENMAX    THKOPT    SHLTHK     SNLOG      ISYM     I2D3D    SLDTHK    SLDSTF 
                                       1 
$     IGAP    IGNORE    DPRFAC    DTSTIF                        FLANGL 
         2 
*CONTACT_... 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*BOUNDARY_PRESCRIBED_MOTION_RIGID 
$   typeID       DOF       VAD      LCID        SF       VID     DEATH     BIRTH 
&bindpid           3         2         3      -1.0         0  
*DEFINE_CURVE 
3 
0.0,0.0 
1.0,&bindmv 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
$ Activate gravity on blank: 
*LOAD_BODY_Z 
90994 
*DEFINE_CURVE_TITLE 
Body Force on blank 
90994   
0.0,9810.0 
10.0,9810.0 
*LOAD_BODY_PARTS 
&blksid 
*END 
Binder closing with real beads example: 
Binder closing with real beads can also be done with implicit static, and with adaptive 
mesh.    An  example  is  shown  in  Figure  12-74,  where  a  hood  outer  is  being  closed 
implicitly.  It is noted a small buckle can be seen near the draw bead region along the 
fender line.  These kind of small forming effects can be more accurately detected with 
implicit static method. 
The implicit static closing can now be set up in LS-PrePost v4.0 Metal Forming 
Application/eZ Setup (http://ftp.lstc.com/anonymous/outgoing/lsprepost/4.0/metal-
forming/). 
Flanging example: 
An  example  of  flanging  simulation  using  this  feature  is  shown  in  Figures  12-75,  12-76 
and  12-77,  with  NUMISHEET’02  fender  outer,  where  flanging  is  conducted  along  the 
hood  line.    A  partial  input  is  provided  below,  where  DTMAX  is  controlled  by  a  load 
curve for contact and speed.  The use of DTMAX with a  load curve is an exception to 
the rule, where most of the time this is not needed.  Smaller step sizes are better in some 
cases than larger step sizes, which may take longer to converge resulting from cutbacks
in  step  sizes.    Gravity,  pad  closing  and  flanging  were  set  to  10%,  10%  and  80%  of  the 
total step size, respectively.  Pad travels a distance of ‘&padtrav’ starting at 0.1, when it 
is  to  be  automatically  moved  to  close  the  gap  with  the  blank  due  to  gravity  loading 
(*CONTACT_AUTO_MOVE),  and  finishing  at  0.2  and  held  in  that  position  until  the 
end.  Flanging steel travels a distance of ‘&flgtrav’ starting at 0.2 and completing at 1.0. 
A detailed section view of the simulation follows in Figure 12-78. 
*KEYWORD 
*PARAMETER ... 
*CONTROL_TERMINATION 
1.0 
*CONTROL_IMPLICIT_FORMING 
$  IOPTION     NSMIN     NSMAX 
         2         2       200 
*CONTROL_IMPLICIT_GENERAL 
         1     0.100 
*CONTROL_IMPLICIT_AUTO 
$    IAUTO    ITEOPT    ITEWIN     DTMIN     DTMAX 
         0         0         0     0.005     -9980 
*DEFINE_CURVE 
9980 
0.0,0.1 
0.1,0.1 
0.2,0.1 
0.7,0.005 
1.0,0.005 
*CONTROL_ADAPTIVE... 
*CONTROL_CONTACT... 
*PART... 
*SECTION_SHELL... 
*CONTACT_... 
*CONTACT_FORMING_SURFACE_TO_SURFACE_ID_MPP 
2 
0,200,,3,2,1.005 
$     SSID      MSID     SSTYP     MSTYP    SBOXID    MBOXID       SPR       MPR 
   &blksid   &padsid         2         2                              
$       FS        FD        DC        VC       VDC    PENCHK        BT        DT 
      0.12       0.0       0.0       0.0      20.0         0       0.0     1E+20 
$      SFS       SFM       SST       MST      SFST      SFMT       FSF       VSF 
       1.0       1.0       0.0     &mstp 
$     SOFT    SOFSCL    LCIDAB    MAXPAR    PENTOL     DEPTH     BSORT    FRCFRQ 
         0 
$   PENMAX    THKOPT    SHLTHK     SNLOG      ISYM     I2D3D    SLDTHK    SLDSTF 
                                       1 
$     IGAP    IGNORE    DPRFAC    DTSTIF                        FLANGL 
         2 
*BOUNDARY_PRESCRIBED_MOTION_RIGID 
$   typeID       DOF       VAD      LCID        SF       VID     DEATH     BIRTH 
   &padpid         3         2         3      -1.0         0  
   &flgpid         3         2         4      -1.0         0  
*DEFINE_CURVE 
3 
0.0,0.0 
0.1,0.0 
0.2,&padtrav 
1.0,&padtrav 
*DEFINE_CURVE 
4 
0.0,0.0 
0.2,0.0 
1.0,&flgtrav 
$ Activate gravity on blank: 
*LOAD_BODY_PARTS
&blksid 
*LOAD_BODY_Z 
90994 
*DEFINE_CURVE_TITLE 
Body Force on blank 
90994   
0.0,9810.0 
10.0,9810.0 
*CONTACT_AUTO_MOVE 
$       ID    ContID       VID      LCID     ATIME 
        -1         2        89         3       0.1 
*END 
Flanging simulation using IOPTION of 1: 
IOPTOIN 1 can also be used for closing and flanging simulation, or other applications 
that  go  through  large plastic  strains  or  deformation.    This  is  used  when  an  equal  step 
size throughout the simulation is desired, and is done by specifying the equal step size 
in  the  variable  DT0  in  *CONTROL_IMPLICIT_GENERAL,  as  shown  in  the  following  
keywords (other cards similar and not included), where DT0 of 0.014 is chosen.  Such an 
application is shown in Figures 12-79 and 12-80. 
*CONTROL_TERMINATION 
1.0 
*CONTROL_IMPLICIT_FORMING 
$  IOPTION 
         1 
*CONTROL_IMPLICIT_GENERAL 
$   IMFLAG       DT0 
         1     0.014 
Switching between implicit dynamic and implicit static for gravity loading: 
For sheet blank gravity loading, it is now possible to start the simulation using implicit 
dynamic  method,  switching  to  implicit  static  method  at  a  user  defined  time  until 
completion.  This feature is activated by setting the variable TDYDTH in *CONTROL_-
IMPLICIT_DYNAMICS  and  was  recently  (Rev.    81400)  linked  together  with  *CON-
TROL_IMPLICIT_FORMING.  In a partial keyword example below, death time for the 
implicit  dynamic  is  set  at  0.55  second.    The  test  model  shown  in  Figure  12-81  (left) 
results in a gravity loaded blank shape in Figure 12-81 (right).  Without the switching, 
the  blank  will  look  like  as  shown  in  Figure  12-82.    The  gravity  loaded  blank  shape  is 
more  reasonable  with  the  switching.    A  check  on  the  energy  history  reveals  that  the 
kinetic energy dissipated completely at 0.60 second, Figure 12-83. 
*CONTROL_TERMINATION 
1.0 
*CONTROL_IMPLICIT_FORMING 
$  IOPTION     NSMIN     NSMAX     BIRTH     DEATH    PENCHK 
         1 
*CONTROL_IMPLICIT_DYNAMICS 
$    IMASS     GAMMA      BETA    TDYBIR    TDYDTH    TDYBUR     IRATE 
         1     0.600     0.380                0.55
Revision information: 
This  implicit  capability  is  available  in  R5.0  and  later  releases.    This  keyword  is 
implemented in LS-PrePost4.0 eZSetup for metal forming application. 
1)Revision 64802: Multi-step gravity loading simulation. 
2)Revision 81400: Switching feature between implicit dynamic and implicit static. 
3)Revision 104837: variable DT0.

Time= 1
Contours of Z-displacement
Original flat sheet blank 
after auto-position
Z-displacement
(mm)
Gravity-loaded blank
Binder opening
Lower binder
7.01
-31.92
-70.86
-109.80
-148.70
-187.70
-226.60
-265.50
-304.50
-343.40
-382.30
Figure  12-69.    Gravity  loading  on  a  box  side  outer  toggle  die  (courtesy  of
Autodie, LLC). 
  Figure 12-70.  Initial auto-positioning (NUMISHEET2005 decklid inner).
Figure 12-71.  At 50% upper travel. 
Figure 12-72.  At 80% upper travel.
Figure 12-73.  Upper travels to home. 
Draw beads
Blank shape upon 
binder closing
Upper cavity
Buckles predicted
Blank
Lower binder (with 
contact offset of 1.1x 
blank thickness)
Figure 12-74.  Binder closing with beads on a hood outer. 
Section A-A
Figure 12-75.  Mean stress at pad closing. 
Figure 12-76.  Mean stress at 40% Travel.
B 
Home (view 1) 
Home (view 2)
Figure 12-77.  Mean stress at flanging home (compression/surface lows in 
red).
Upper pad
Flanging 
post
Trimmed 
panel
Flanging 
steel
 Figure 12-78.  Flanging progression along section B (flanging post stationary).
Thinning (%)
20.0
18.0
16.0
14.0
12.0
10.0
8.0
6.0
4.0
2.0
 0.0
Flanged area in detail next figure
Figure  12-79.    Flanging  simulation  of  a  rear  floor  pan  using  IOPTION  1
(Courtesy of Chrysler, LLC). 
Thinning (%)
20.0
Pressure (MPa)
294.1
18.0
16.0
14.0
12.0
10.0
8.0
6.0
4.0
2.0
-0.0
Thinning contour
235.9
177.7
119.5
61.25
3.03
-55.2
-113.4
-171.6
-229.8
-288.1
Mean stress contour - 
compression in red
Figure 12-80.  Localized view of the last figure.
Initial totally flat 
sheet blank
Binder
Time=0
Time=1.0
Figure  12-81.    Test  model  (left)  and  gravity  loaded  blank  (right)  with
switching from implicit dynamic to implicit static. 
Figure 12-82.  Gravity loaded blank without the “switching”. 
Time=1.0
25
20
15
10
)
(
0.0
t=0.55 t=0.60
Implicit dynamic
Implicit static
Kinetic energy
Internal energy
Total energy
Kinetic energy dissipates 
after a small transition step
0.2
0.4
0.6
0.8
1.0
Implicit "time" (sec.)
Figure 12-83.  Switching between implicit dynamic and implicit static.
*CONTROL_IMPLICIT_GENERAL_{OPTION} 
Availlable option s include: 
<BLANK> 
DYN 
SPR 
Purpose:    Activate  implicit  analysis  and  define  associated  control  parameters.    This 
keyword is required for all implicit analyses.  The  DYN option allows setting controls 
specifically  for  the  dynamic  relaxation  phase.    The  SPR  option  allows  setting  controls 
specifically for the springback phase. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IMFLAG 
DT0 
IMFORM 
NSBS 
IGS 
CNSTN 
FORM 
ZERO_V 
Type 
Default 
I 
0 
F 
none 
I 
2 
I 
1 
I 
2 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
IMFLAG 
Implicit/Explicit analysis type flag 
EQ.0: explicit analysis 
EQ.1: implicit analysis 
EQ.2: explicit followed by implicit, (seamless springback).  *IN-
to 
is  required 
TERFACE_SPRINGBACK_SEAMLESS 
activate seamless springback. 
EQ.4: implicit with automatic implicit-explicit switching 
EQ.5: implicit  with  automatic  switching  and  mandatory
implicit finish 
EQ.6: explicit with intermittent eigenvalue extraction 
LT.0:  curve ID = -IMGFLAG specifies IMFLAG as a function of 
time. 
DT0 
Initial time step size for implicit analysis
Implicit 1
Explicit 0
 Figure 12-84.  Solution method, implicit or explicit, controlled by a load curve.
Time
  VARIABLE   
IMFORM 
DESCRIPTION
Element  formulation  flag  for  seamless  springback;  see  *INTER-
FACE_SPRINGBACK_SEAMLESS. 
EQ.1: switch 
to 
springback 
fully 
integrated  shell 
formulation 
for
EQ.2: retain original element formulation (default) 
NSBS 
Number  of  implicit  steps  in  seamless  springback;  see  *INTER-
FACE_SPRINGBACK_SEAMLESS. 
IGS 
Geometric (initial stress) stiffness flag 
EQ.1: include 
EQ.2: ignore 
CNSTN 
Indicator  for  consistent  tangent  stiffness  (solid  materials  3  &  115
only): 
EQ.0: do not use (default) 
EQ.1: use. 
FORM 
integrated  element 
Fully 
IMFORM = 1 only) 
formulation 
(IMFLAG = 2  and 
EQ.0: type 16 
EQ.1: type 6.
VARIABLE   
DESCRIPTION
ZERO_V 
Zero out the velocity before switching from explicit to implicit. 
EQ.0: The velocities are not zeroed out. 
EQ.1: The velocities are set to zero. 
Remarks: 
  VARIABLE   
IMFLAG 
REMARK
The  default  value  0  indicates  a  standard  explicit  analysis  will  be
performed.    Using  value  1  causes an  entirely  implicit  analysis  to
be  performed.    Value  2  is  automatically  activated  when  the
keyword  *INTERFACE_SPRINGBACK_SEAMLESS  is  present, 
causing the analysis type to switch from explicit to implicit when
the  termination  time  is  reached.    Other  nonzero  values  for  IM-
FLAG  can  also  be  used  with  *INTERFACE_SPRINGBACK_-
SEAMLESS.    After  this  switch,  the  termination  time  is  extended
by  NSBS*DT0,  or  reset  to  twice  its  original  value  if  DT0 = 0.0.    The 
implicit simulation then proceeds until the new termination time
is  reached.    Contact  interfaces  are  automatically  disabled  during
the implicit phase of seamless springback analysis.  Furthermore,
implicit  stabilization  (*CONTROL_IMPLICIT_STABILIZATION) 
and automatic step size adjustment (*CONTROL_IMPLICIT_AU-
TO) on by default for seamless springback. 
When the automatic implicit-explicit switching option is activated 
(IMFLAG = 4 or 5), the solution method will begin as implicit.  If 
convergence  of  the  equilibrium  iterations  fails,  the  solution  will
automatically switch to explicit for a time interval of DTEXP .    After  this  time  interval,  the 
solution  method  will  switch  back  to  implicit  and  attempt  to
proceed.  The implicit simulation may be either static or dynamic.
When this feature is used in a static implicit job, simulation time
is no longer arbitrary, and must be chosen along with DTEXP in a 
realistic  way  to  allow  efficient  execution  of  any  explicit  phases.
Mass scaling may also be activated , 
and will apply only during the explicit phases of the calculation.
In  cases  where  much  switching  occurs,  users  must  exercise
caution  to  ensure  that  negligible  dynamic  effects  are  introduced
by the explicit phases. 
When  IMFLAG = 5,  the  final  step  of  the  simulation  must  be
implicit.  The termination time will be extended automatically as
necessary,  until  a  successfully  converged  implicit  step  can  be
VARIABLE   
REMARK
obtained.    This  is  useful  for  example  in  difficult  metal  forming
springback simulations. 
When  IMFLAG = 6,  an  explicit  simulation  will  be  performed.
Eigenvalues will be extracted intermittently according to a curve
indicated  by  NEIG=(-curve  ID)  on  *CONTROL_IMPLICIT_-
EIGENVALUE.    Beware  that  dynamic  stress  oscillations  which
may occur in the explicit simulation will influence the geometric
(initial  stress)  stiffness  terms  used 
in  the  eigen  solution,
potentially producing misleading results and/or spurious modes. 
As an alternative, eigenvalues can also be extracted intermittently
during an implicit analysis, using IMFLAG = 1 and NEIG=(-curve 
ID). 
When  IMFLAG < 0,  a  curve  ID  is  indicated  which  gives  the
solution  method  as  a  function  of  time.    Define  a  curve  value  of 
zero  during  explicit  phases,  and  a  value  of  one  during  implicit
phases.    Use  steeply  sloping  sections  between  phases.    An
arbitrary  number  of formulation  switches  may  be  activated  with
this method.  See Figure 12-84. 
This  parameter  selects  the  initial  time  step  size  for  the  implicit
phase  of  a  simulation.    The  step  size  may  change  during  a
multiple  step  simulation  if  the  automatic  time  step  size  control
feature is active  
Adaptive  mesh  must  be  activated  when  using  element
formulation switching.  For best springback accuracy, use of shell
type  16  is  recommended  during  the  entire  stamping  and
springback  analysis,  in  spite  of  the  increased  cost  of  using  this
element during the explicit stamping phase. 
The  NSBS  option  allows  a  seamless  springback  analysis,  invoked
with  *INTERFACE_SPRINGBACK_SEAMLESS,  to  use  multiple 
unloading  steps.    Implicit  seamless  springback  beings  at  time,
𝑡 = ENDTIM  and  finishes  at  𝑡 = ENDTIM + NSBS × DT0  were 
ENDTIM is specified in *CONTROL_TERMINATION and DT0 is 
specified in *CONTROL_IMPLICIT_GENERAL. 
The  geometric  stiffness  adds  the  effect  of  initial  stress  to  the
global stiffness matrix.  This effect is seen in a piano string whose
natural frequency changes with tension.  Geometric stiffness does
not  always  improve  nonlinear  convergence,  especially  when
DT0 
INFORM 
NSBS 
IGS
VARIABLE   
REMARK
compressive  stresses  are  present,  so  its  inclusion  is  optional.
Furthermore,  the  geometric  stiffness  may  lead  to  convergence
incompressible,
incompressible,  or  nearly 
problems  with 
materials.
*CONTROL_IMPLICIT_INERTIA_RELIEF 
Purpose:  Allows analysis of linear static problems that have rigid body modes. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IRFLAG 
THRESH 
IRCNT 
Type 
Default 
I 
0 
F 
0.001 
I 
0 
Additional Mode List  Cards.  This card should be included only when the user wants 
to  specify  the  modes  to  use.    Include  as  many  cards  as  needed  to  provide  all  values. 
This input ends at the next keyword (“*”) card.  The mode numbers do not have to be 
consecutive. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MODE1  MODE2  MODE3  MODE4  MODE5  MODE6  MODE7  MODE8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
IRFLAG 
Inertia relief flag 
EQ.0: do not perform inertia relief 
EQ.1: do perform inertia relief 
THRESH 
Threshold  for  what  is  a  rigid  body  mode.    The  default  is  set  to
0.001 Hertz where it is assumed that the units are in seconds. 
IRCNT 
MODEi 
The  user  can  specify  to  use  the  lowest  IRCNT  modes  instead  of
using THRESH to determine the number of modes. 
Ignore  THRESH  and  IRCNT  and  use  a  specific  list  of  modes,
skipping those that should not be used.
*CONTROL 
Purpose:  Specify penalty or constraint treatment of joints for implicit analysis. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ISPHER 
IREVOL 
ICYLIN 
Type 
Default 
I 
1 
I 
1 
I 
1 
  VARIABLE   
DESCRIPTION
ISPHER 
Treatment of spherical joints 
EQ.1: use constraint method for all spherical joints (default) 
EQ.2: use penalty method for all spherical joints 
IREVOL 
Treatment of revolute joints 
EQ.1: use constraint method for all revolute joints (default) 
EQ.2: use penalty method for all revolute joints 
ICYLIN 
Treatment of cylindrical joints 
EQ.1: use constraint method for all cylindrical joints (default) 
EQ.2: use penalty method for all cylindrical joints 
Remarks: 
For  most  implicit  applications  one  should  use  the  constraint  (default)  method  for  the 
treatment of joints.  When explicit-implicit switching is used the joint treatment should 
be  consistent.    This  keyword  allows  the  user  to  choose  the  appropriate  treatment  for 
their application.
*CONTROL_IMPLICIT_MODAL_DYNAMIC 
Purpose:  Activate implicit modal dynamic analysis.  Eigenmodes are used to linearize 
the  model  by  projecting  the  model  onto  the  space  defined  by  the  eigenmodes.    The 
eigenmodes can be computed or read from a file.  All or some of the modes can be used 
in the linearization.  Modal damping can be applied.   
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MDFLAG 
ZETA 
Type 
I 
F 
Optional Filename Card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
FILENAME 
A80 
  VARIABLE   
DESCRIPTION
MDFLAG 
Modal Dynamic flag 
EQ.0:  no modal dynamic analysis 
EQ.1:  perform modal dynamic analysis. 
ZETA 
Modal Dynamic damping constant. 
FILENAME 
If  specified  the  eigenmodes  are  read  from  the  specified  file.
Otherwise  the  eigenmodes  are  computed  as  specified  on  *CON-
TROL_IMPLICIT_EIGENVALUE. 
Remarks: 
Modal  Dynamic  uses  the  space  spanned  by  the  eigenmodes  of  the  generalized 
eigenvalue problem 
The matrix of eigenmodes, 𝚽, diagonalizes  𝐊 and 𝐌 
𝐊𝛟𝑖 = 𝜆𝑖𝐌𝛟𝑖. 
𝚽𝐓𝐊𝚽 = 𝚲
and 
 𝚽𝐓𝐌𝚽 = 𝐈. 
Multiplication  by  𝜱  changes  coordinates  from  amplitude  space  to  displacement  space 
as 
where 𝒂 is a vector of modal amplitudes.  The equations of motion  
𝐌𝐮̈𝑛+1 + 𝐊𝚫𝐮 = 𝐅(𝐱𝒏) 
𝐮 = 𝚽𝐚 
when  multiplied  on  the  left  by  𝛟T  and  substituting  𝐮 = 𝚽𝐚  become  the  linearized 
equations of motion in its spectral form as, 
𝐈𝐚̈𝑛+1 + 𝚲(𝚫𝐚) = 𝚽T𝐅(𝐱𝑛). 
The modal damping features adds a velocity dependent damping term, 
𝐈𝐚̈𝑛+1 + 2𝐙𝐚̇𝑛 + 𝚲(𝚫𝐚) = 𝚽T𝐅(𝐱𝒏) 
Where 𝑍𝑖𝑖 = 𝜁𝑖𝜔𝑖, 𝜔𝑖 = √𝜆𝑖, and each 𝜁𝑖 is a user specified damping coefficients. 
The matrices in the reduced equations are diagonal and constant.  So Modal Dynamics 
can  quickly  compute  the  acceleration  of  the  amplitudes  and  hence  the  motion  of  the 
model.  But the motion is restricted to the space spanned by the eigenmodes. 
Eigenmodes  are  either  computed  based  on  *CONTROL_IMPLICIT_EIGENVALUE  or 
read  from  file  FILENAME.    By  default  all  modes  are  used  in  the  projection.    Selected 
modes  can  be  specified  via  *CONTROL_IMPLICIT_MODAL_DYNAMIC_MODE  to 
reduce the size of the projection.  .  
Stresses are computed only for linear shell formulation 18 and linear solid formulation 
18. 
Modal damping on all modes can be specified using ZETA.  More options for specifying 
modal damping can be found on *CONTROL_IMPLICIT_MODAL_DYNAMIC_DAMP-
ING. 
Using MDFLAG = 1, ZETA = 0.0, and FILENAME = “ ” is the same as using IMASS = 2 
with *CONTROL_IMPLICIT_DYNAMICS.  Using MDFLAG = 1, ZETA = 0.0 and FILE-
NAME = ’d3eigv’ is the same as IMASS = 3.  The new keywords *CONTROL_IMPLIC-
IT_MODAL_DYNAMIC_MODE  and  *CONTROL_IMPLICIT_MODAL_DYNAMIC_-
DAMPING provide additional user options for mode selection and modal damping.
*CONTROL_IMPLICIT_MODAL_DYNAMIC_DAMPING_{OPTION} 
Available options include: 
BLANK 
SPECIFIC 
FREQUENCY_RANGE 
Purpose:  Define vibration modes to be used in implicit modal dynamic.  
Damping Card.  Card for option set to <BLANK>. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ZETA1 
Type 
F 
I 
Specific Damping Cards.  Cards for the SPECIFIC option.  This input ends at the next 
keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID1 
ZETA1 
MID2 
ZETA2 
MID3 
ZETA3 
MID4 
ZETA4 
Type 
I 
F 
I 
F 
I 
F 
I 
F 
Frequency  Range  Damping  Cards.    Cards  for  FREQUENCY_RANGE  option.    This 
input ends at the next keyword (“*”) card.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FREQ1 
ZETA1 
FREQ2 
ZETA2 
FREQ3 
ZETA3 
FREQ4 
ZETA4 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
VARIABLE 
DESCRIPTION 
ZETAn 
Modal Dynamic damping coefficient n. 
MIDn 
Mode ID n.
f1
f2 f3
f4
f5
frequency
Figure 12-85.  Schematic illustration of frequency range damping. 
VARIABLE 
DESCRIPTION 
FREQn 
Frequency value n. 
Remarks: 
1. 
2. 
3. 
If  no  option  is  specified  the  value  of  ZETA1  becomes  the  damping  coefficient 
for  all  modes  involved  in  implicit  modal  dynamic  analysis.    This  value  over-
rides the value on *CONTROL_IMPLICIT_MODAL_DYNAMIC. 
If  option  SPECIFIC  is  specified  the  integers  MIDn  indicate  which  modes 
involved  in  *CONTROL_IMPLICIT_MODAL_DYNAMIC  will  have  modal 
damping  applied  to  them.    The  associated  value  ZETAn  will  be  the  modal 
damping coefficient for that mode. 
If option FREQUENCY_RANGE is specified all modes involve will have modal 
damping applied.  The damping coefficient will be computed by linear interpo-
lation of the pairs (FREQi, ZETAi).  If the modal frequency is less than FREQ1 
then the modal damping coefficient will be  ZETA1.  If the modal  frequency is 
greater  than  FREQn  then  the  modal  damping  coefficient  will  be  ZETAn.    The 
values of FREQi must be specified in ascending order.
*CONTROL_IMPLICIT_MODAL_DYNAMIC_MODE_OPTION 
Available options include: 
LIST 
GENERATE 
Purpose:  Define vibration modes to be used in implicit modal dynamic. 
Mode  ID  Cards.    Card  1  for  the  LIST  keyword  option.    For  each  mode  include  an 
addition.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID1 
MID2 
MID3 
MID4 
MID5 
MID6 
MID7 
MID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Mode Range Cards.  Card 1 for the GENERATE keyword option.  For each range of 
modes include an additional card.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  M1BEG  M1END  M2BEG  M2END  M3BEG  M3END  M4BEG  M4END 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
MIDn 
Mode ID n. 
MnBEG 
First mode ID in block n. 
MnEND 
Last  mode  ID  in  block  n.    All  mode  ID’s  between  and  including 
MnBEG and MnEND are added to the list. 
Remarks: 
1.  User may use this keyword with *CONTROL_IMPLICIT_MODAL_DYNAMIC 
if  some  of  the  vibration  modes  have  less  contribution  to  the  total  structural 
response and can be removed from the implicit modal dynamic analysis.
*CONTROL_IMPLICIT_MODES_{OPTION} 
Available options include: 
<BLANK> 
BINARY 
Purpose:    Request  calculation  of  constraint,  attachment,  and/or  eigenmodes  for  later 
use in modal analysis using *PART_MODES  or *ELEMENT_DIRECT_MATRIX_INPUT. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSIDC 
NSIDA 
NEIG 
IBASE 
SE_MASS SE_DAMP  SE_STIFF  SE_INERT
I 
0 
2 
Type 
Default 
I 
0 
  Card 2 
1 
Variable 
Type 
I 
I 
C 
C 
C 
C 
3 
4 
5 
6 
7 
8 
SE_FILENAME 
C 
  VARIABLE 
DESCRIPTION
NSIDC 
Node set ID for constraint modes 
EQ.0: no constraint modes will be generated 
NSIDA 
Node set ID for attachment modes 
EQ.0: no attachment modes will be generated 
NEIG 
Number of eigenmodes (normal modes) 
EQ.0: no eigenmodes will be generated 
IBASE 
Offset  for  numbering  of  the  generalized  internal  degrees  of
freedom for the superelement
SE_MASS 
*CONTROL_IMPLICIT_MODES 
DESCRIPTION
Name  of  the  superelement  mass  matrix.    If  left  blank  it  is  not 
generated. 
SE_DAMP 
Name of the superelement damping matrix.  If left blank it is not
generated. 
SE_STIFF 
Name of the superelement stiffness matrix.  If left blank it is not
generated. 
SE_INERT 
Name  of  the  superelement  inertia  matrix,  required  for  gravity
loading  applications  of  the  superelement.    If  left  blank  it  is  not
generated. 
SE_FILENAME 
If  any  of  SE_MASS,  SE_DAMP,  SE_STIFF,  or  SE_INERT  are  not 
blank then the second line is required and contains the file name 
for the superelement. 
Remarks: 
To use this feature, an implicit analysis must be requested using IMFLAG = 1 on *CON-
TROL_IMPLICIT_GENERAL,  and  a  non-zero  termination  time  must  be  specified  on 
*CONTROL_TERMINATION.  A double precision version of LS-DYNA should be used 
for best accuracy.  Care must be taken to apply a sufficient number of constraints to the 
model  to  eliminate  static  rigid  body  motion.    Computed  modes  are  written  to  binary 
output  file  d3mode,  with  the  order  of  output  being  constraint  modes,  followed  by 
attachment  modes,  and  then  eigenmodes.    The  d3mode  file  can  be  read  and  modes 
viewed using LS-PrePost.  Eigenmodes  are also written to binary output file d3eigv. 
Constraint  and  attachment  modes  are  generated  by  applying  unit  displacements  and 
unit  forces,  respectively,  to  each  specified  degree  of  freedom.    By  default,  modes  are 
computed for all degrees of freedom for each node in sets NSIDC and NSIDA.  The first 
and  second  node  set  attribute  parameters  can  be  optionally  used  to  restrict  the 
translational  and  rotational  degrees  of  freedom  for  which  modes  are  requested, 
respectively, according to the following syntax: 
Node set attribute parameters DA1 and A1:  translational degree of freedom codes 
Node set attribute parameters DA2 and A2:  rotational degree of freedom codes 
code  modes computed 
 
X degree of freedom only 
Y degree of freedom only 
0 
1
3 
4 
5 
6 
7 
Z degree of freedom only 
X, Y degrees of freedom only 
Y, Z degrees of freedom only 
X, Z degrees of freedom only 
X, Y, Z degrees of freedom 
Setting both node set attributes to zero is equivalent to setting both node set attributes 
to 7 (X, Y, and Z for translational and rotational degrees of freedom). 
If one node set attribute is nonzero (codes 1 to 7) and the other node set attribute is zero, 
then the zero attribute means  NO degrees of freedom are considered.  For example, if 
DA1 = 2  and  DA2 = 0,  then  only  the  Y-translational  degree  of  freedom  modes  are 
calculated. 
Eigenmodes  are  generated  for  the  model  with  single  point  constraints  applied  on  the 
constraint  modes.    The  number  of  eigenmodes  is  specified  here.    If  the  user  wants  to 
compute eigenmodes other than the lowest ones, the controls on *CONTROL_IMPLIC-
IT_EIGENVALUE can be used. 
When  the  superelement  is  created  an  internal  numbering  must  be  applied  to  the 
attachment and eigen modes.  This numbering starts at IBASE+1. 
The user can create the superelement representation of the reduced model by specifying 
the SE_MASS, SE_DAMP, SE_STIFF, SE_INERT and SE_FILENAME fields.  The inertia 
matrix is necessary if  body forces, e.g., gravity loads, are applied to the superelement.  
The file, by default is written in the Nastran DMIG file format and can be used as input 
to  *ELEMENT_DIRECT_MATRIX_INPUT.    The  BINARY  keyword  option  can  be  used 
to  create  a  binary  representation  for  the  superelement  which  can  be  used  with  *ELE-
MENT_DIRECT_MATRIX_INPUT_BINARY to reduce the file size. 
The combination of constraint modes and eigenmodes form the Hurty-Craig-Bampton 
linearization  for  a  model.    Using  only  constraint  modes  is  the  same  as  static 
condensation. 
Some  broad  guidelines  for  appropriate  selection  of  constraint  modes,  attachment 
modes, and eigenmodes include: 
1.  Use  constraint  modes  for  the  nodal  degrees-of-freedom  that  are  to  be  "con-
strained" with SPCs or prescribed motion. 
2.  Use  attachment  modes  for  nodal  degrees-of-freedom  that  are  under  the 
influence of point loads.
3.  Use eigenmodes in the construction of the superelement to capture the reaction 
of the part being modeled by the superelement and the associated feedback to 
the rest of the model.
*CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS 
Purpose:    This  keyword  is  used  to  model  rotational  dynamics  using  the  implicit  time 
integrator.  Applications for this feature include the transient and vibration analysis of 
rotating  parts  such  as  turbine  blades,  propellers  in  aircraft,  and  rotating  disks  in  hard 
disk  drives.    The  current  implementation  requires  a  double-precession  SMP  version  of 
LS-DYNA.  An MPP implementation is under development. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
STYPE 
OMEGA 
VID 
NOMEG 
IREF 
OMEGADR 
Type 
I 
Default 
none 
I 
0 
F 
I 
none 
none 
I 
0 
I 
0 
F 
0 
Additional  Rotational  Speed  Cards.    This  card  should  be  included  only  when 
NOMEG > 0.    Include  as  many  cards  as  needed  to  provide  all  NOMEG  values.    This 
input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OMEG1 
OMEG2 
OMEG3 
OMEG4 
OMEG5 
OMEG6 
OMEG7 
OMEG8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
SID 
Set ID of the rotational components. 
STYPE 
Set type: 
EQ.0: Part; 
EQ.1: Part set. 
OMEGA 
Rotating speed. 
GT.0: rotating speed. 
LT.0:  curve ID = (-OMEGA) gives rotating speed as a function 
of time.
VID 
*CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS 
DESCRIPTION
Vector  ID  to  define  the  rotating  axis.    It  can  be  defined  in  *DE-
FINE_VECTOR  and  *DEFINE_VECTOR_NODES,  and  the  tail  of 
the vector should be set as the rotating center. 
NOMEG 
Number  of  rotating  speeds. 
  This  feature  is  intended  to
automatically  preform  parameter  studies  with  respect  to  the
rotation  speed.    The  keyword  *CONTROL_IMPLICIT_EIGEN-
VALUE must be included if NOMEG > 0. 
IREF 
Reference frame: 
EQ.0: Rotating  coordinate  system  and  rotating  parts  will  not 
rotate  in  visualization.    Solid  element  and  thick  shell
element will use IREF = 0. 
EQ.1: Fixed  coordinate  system.    Rotating  parts rotates  and  the
initial rotating velocity should be defined in *INITIAL_-
VELOCITY_GENERATION as well. 
EQ.2: Rotating  coordinate  system,  but  rotate  rotating  parts  for
visualization purpose. 
OMEGn 
The nth rotating speed. 
OMEGADR 
Rotating speed defined in dynamic relaxation. 
GT.0: rotating speed defined in dynamic relaxation. 
LT.0:  curve ID = (-OMEGA) gives rotating speed as a function 
of  time. 
Remarks: 
The linearized equilibrium equation in the rotating coordinate system is given by 
Whereas, in a fixed coordinate system, the linearized equilibrium equation is 
𝐌𝐮̈ + (𝐃 + 2Ω𝐂)𝒖̇ + (𝑲 − Ω2𝐊𝐺)𝐮 = 𝐅 
𝐌𝐮̈ + (𝐃 + Ω𝐂)𝐮̇ + 𝐊𝐮 = 𝐅 
with 
𝐌 = lumped mass matrix 
𝐃 = damping matrix 
𝐊 = stiffness matrix 
𝐂 = gyroscopic matrix
𝐊𝐺 = centrifugal stiffness matrix 
𝐮 = nodal displacement vector 
𝐮̇ = nodal point velocities at time  
𝐮̈ = nodal point acceleration at time 
Ω = rotating speed 
The  chief  difference  between  the  equations  for  the  rotating  and  fixed  frames  is  the 
inclusion  of  the  centrifugal  stiffness  matrices𝐊𝑔.    Additionally,  the  coefficient  on  the 
gyroscopic  matrix,  𝐂,  as  well  as  its  content  are  modified  in  the  rotating-frame  case.  
Specifically, the rotating system includes an additional Coriolis contribution to 𝐂. 
In many applications of rotational dynamics, the critical speed – the theoretical angular 
velocity that excites the natural frequency of a rotating object – is of particular concern.  
Therefore, the study of mode frequency response with the change of the rotating speed 
is  very  important.    The  Campbell  diagram,  which  is  defined  to  represent  a  system’s 
eigen-frequencies  as  a  function  of  rotating  speeds,  is  introduced  for  this  purpose.    In 
order  to  do  this,  the  user  needs  to  define  a  set  of  rotating  speeds  on  card  2,  and  LS-
DYNA will do modal analysis for each of these speeds.  NOMEG should be defined as 
the  number  of  rotating  speeds  used  in  card  2.    A  keyword  file  example  in  this 
application can be set as follows: 
*KEYWORD 
*CONTROL_TERMINATION... 
*CONTROL_IMPLICIT_EIGENVALUE 
         5 
*CONTROL_IMPLICIT_GENERAL 
         1      0.05 
*CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS 
$#     SID     STYPE     OMEGA       VID    NOMEGA      IREF   
         1         0       0.0         1         4         1 
$#   OMEG1     OMEG2     OMEG3     OMEG4 
      50.0     100.0     150.0     200.0 
*DEFINE_VECTOR 
$#     VID        XT        YT        ZT        XH        YH        ZH       CID 
         1       0.0       0.0       0.0       1.0       0.0       0.0         
*DATABASE_... 
*PART... 
*SECTION... 
*MAT... 
*ELEMENT... 
*NODE... 
*END 
Besides  of  modal  analysis,  transient  analysis  can  also  be  done  using  this  keyword.    A 
keyword file example can be set as follows: 
*KEYWORD 
*CONTROL_TERMINATION... 
*CONTROL_IMPLICIT_GENERAL 
         1      0.05 
*CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS 
$#     SID     STYPE     OMEGA       VID    NOMEGA      IREF   
         1         0       0.0         1         0         0
*DEFINE_VECTOR 
$#     VID        XT        YT        ZT        XH        YH        ZH       CID 
         1       0.0       0.0       0.0       1.0       0.0       0.0         
*DATABASE_... 
*PART... 
*SECTION... 
*MAT... 
*ELEMENT... 
*NODE... 
*END
*CONTROL_IMPLICIT_SOLUTION_{OPTION} 
Available options include: 
<BLANK> 
DYN 
SPR 
Purpose:  These optional cards apply to implicit calculations.  Use these cards to specify 
whether  a  linear  or  nonlinear  solution  is  desired.    Parameters  are  also  available  to 
control the  implicit  nonlinear  and  arc  length  solution  methods  .    The  DYN  option  allows  setting  controls  specifically  for  the 
dynamic  relaxation  phase.    The  SPR  option  allows  setting  controls  specifically  for  the 
springback phase. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSOLVR 
ILIMIT  MAXREF 
DCTOL 
ECTOL 
RCTOL 
LSTOL 
ABSTOL 
Type 
I 
I 
I 
F 
F 
F 
F 
F 
Default 
12 
11 
15 
0.001 
0.01 
1010 
0.90 
10-10 
Remaining cards are optional.† 
 Optional 
2a 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DNORM 
DIVERG 
ISTIF 
NLPRINT  NLNORM D3ITCTL 
CPCHK 
Type 
Default 
I 
2 
I 
1 
I 
1 
I 
0 
F/I 
2 
I 
0 
I 
0 
Strict Tolerances Optional Card.  Define this card if and only if DNORM.LT.0
Optional 
2b 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DMTOL 
EMTOL 
RMTOL 
NTTOL 
NRTOL 
RTTOL 
RRTOL 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Arc Length Optional Card.  The contents of this card are ignored unless an arc-length 
method is activated (6 ≤ NSOLVR ≤ 9, or NSOLVR = 12 and ARCMTH = 3). 
Optional 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ARCCTL 
ARCDIR 
ARCLEN  ARCMTH  ARCDMP 
ARCPSI 
ARCALF 
ARCTIM 
Type 
Default 
I 
0 
I 
none 
F 
0 
I 
1 
I 
2 
F 
0. 
F 
0. 
F 
0. 
Line Search Parameter Optional Card. 
Optional 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LSMTD 
LSDIR 
IRAD 
SRAD 
AWGT 
SRED 
Type 
Default 
I 
4 
I 
2 
F 
F 
F 
F 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
NSOLVR 
Solution method for implicit analysis: 
EQ.1:  Linear 
EQ.12:  Nonlinear  with  BFGS  updates  +  optional  arclength,
(default)    incorporating  different  line  search  and  inte-
gration schemes compared to solver 2. 
EQ.2:  Nonlinear with BFGS updates (obsolete)
VARIABLE   
DESCRIPTION
EQ.3:  Nonlinear with Broyden updates 
EQ.4:  Nonlinear with DFP updates 
EQ.5:  Nonlinear with Davidon updates 
EQ.6:  Nonlinear with BFGS updates + arclength 
EQ.7:  Nonlinear with Broyden updates + arclength 
EQ.8:  Nonlinear with DFP updates + arclength 
EQ.9:  Nonlinear with Davidon updates + arclength 
ILIMIT 
Iteration limit between automatic stiffness reformations 
MAXREF 
Stiffness reformation limit per time step. 
LT.0:  If |MAXREF| matrix reformations occur convergence for
that time step is forced, see REMARKS. 
DCTOL 
Displacement relative convergence tolerance 
ECTOL 
Energy relative convergence tolerance 
RCTOL 
Residual  (force)  relative  convergence  tolerance  (DEFAULT = 
inactive) 
LSTOL 
Line search convergence tolerance 
ABSTOL 
Absolute convergence tolerance. 
LT.0:  Convergence  detected  when  the  residual  norm  is  less
than  –ABSTOL  (Tip:  To  drive  convergence  based  on  –
ABSTOL, set DCTOL and ECTOL to 1.0E-20) 
DNORM 
Displacement norm for convergence test 
EQ.1:  Increment vs.  displacement over current step 
EQ.2:  Increment vs.  total displacement (default) 
If DNORM.LT.0, this is to be interpreted as its absolute value, but
activates reading of optional card 2b. 
DIVERG 
Divergence  flag  (force  imbalance  increase  during  equilibrium
iterations) 
EQ.1:  reform stiffness if divergence detected (default)
VARIABLE   
DESCRIPTION
EQ.2:  ignore divergence 
ISTIF 
Initial stiffness formation flag 
EQ.1:  reform stiffness at start of each step (default) 
EQ.n:  reform stiffness at start of every “n”th step 
NLPRINT 
Nonlinear solver print flag 
EQ.0:  no  nonlinear  iteration  information  printed  (new  v970
default) 
EQ.1:  print  iteration  information  to  screen,  message,  d3hsp
files 
EQ.2:  print extra norm information (NLNORM = 1) 
EQ.3:  same as 2, but also print information from line search 
  NOTE: during execution, interactive commands can be used: 
response 
toggle NLPRINT between 0 and 1 
toggle NLPRINT between 0 and 2 
interactive command 
<ctrl-c> nlprint   
<ctrl-c> diagnostic 
<ctrl-c> information 
set NLPRINT = 2 for one iteration 
NLNORM 
Nonlinear  convergence  norm  type,  input  an  integer  if  zero  or  a
positive number is used and float if a negative value is used 
LT.0:  Same  as  4,  but  rotational  degrees  of  freedom  are  scaled
appropriately  with  characteristic  length  |NLNORM|  to
account for units.  See remarks. 
EQ.1:  consider translational and rotational degrees of freedom
EQ.2:  consider translational degrees of freedom only (default) 
EQ.4:  consider  sum  of  translational  and  rotational  degrees  of
freedom, i.e., no separate treatment.  See remarks. 
D3ITCTL 
Control d3iter database.  If nonzero, the search directions for the
nonlinear implicit solution are written to the d3iter database.  To 
reduce the size of the d3iter database the database is reset every n 
time steps where n = d3itctl. 
CPCHK 
Contact  penetration  check  flag.    This  flag  does  not  apply  to
mortar contacts. 
EQ.0:  no contact penetration check is performed (default).
VARIABLE   
DESCRIPTION
DMTOL 
EMTOL 
RMTOL 
NTTOL 
NRTOL 
RTTOL 
RRTOL 
EQ.1:  check  for  contact  penetration  during  the  nonlinear
solution procedure.  If such penetration is found modify
the line search to prevent unnecessary penetration. 
Maximum  displacement  convergence  tolerance,  convergence  is
detected  when  the  relative  maximum  nodal  or  rigid  body 
displacement is less than this value  
Maximum energy convergence tolerance, convergence is detected
when the relative maximum nodal or rigid body energy increment
is less than this value  
is
Maximum  residual  convergence 
detected when the relative maximum nodal or rigid body residual 
is less than this value 
tolerance,  convergence 
translational  convergence 
is
Nodal 
detected when the absolute maximum nodal translational residual 
is less than this value 
tolerance,  convergence 
Nodal  rotational  convergence  tolerance,  convergence  is  detected
when the absolute maximum nodal rotational residual is less than
this value 
Rigid  body  translational  convergence  tolerance,  convergence  is
detected  when  the  absolute  maximum  rigid  body  translational 
residual is less than this value 
Rigid  body  rotational  convergence  tolerance,  convergence  is
detected  when  the  absolute  maximum  rigid  body  rotational 
residual is less than this value 
ARCLEN 
Relative arc length size.  See remarks below. 
LE.0.0:  use automatic size, 
GT.0.0:  use ARCLEN × (automatic step size). 
ARCMTH 
Arc length method 
EQ.1:  Crisfield (default) 
EQ.2:  Ramm 
EQ.3:  Modified Crisfield (used with NSOLVR = 12 only) 
ARCDMP 
Arc length damping option
VARIABLE   
DESCRIPTION
EQ.2:  off (default) 
EQ.1:  on, oscillations in static solution are suppressed 
ARCPSI 
ARCALF 
Relative  influence  of  load/time  parameter  in  spherical  arclength
constraint,  default  value  is  0  which  corresponds  to  a  cylindrical
arclength constraint.  Applies to ARCMTH = 3. 
Relative  influence  of  predictor  step  direction  for  positioning  of
the  arc  center,  default  is  0  which  means  that  the  center  is  at  the
origin.  Applies to ARCMTH = 3. 
ARCTIM 
Optional  time  when  arclength  method  is  initiated.    Applies  to
ARCMTH = 3. 
LSMTD 
Line search convergence method: 
EQ.1:  Energy method using only translational variables 
EQ.2:  Residual method 
EQ.3:  Energy  method  using  both  translational  and  rotational
variables 
EQ.4:  Energy method using sum of translational and rotational
degrees of freedom (default), i.e., no separate treatment 
EQ.5:  Same  as  4,  but  account  for  residual  norm  growth  to  be 
extra conservative in step length  
EQ.6:  Same  as  5,  but  minimizes  the  residual  norm  whenever
convenient. 
LSDIR 
Line search direction method: 
EQ.1:  Search  on  all  variables  (traditional  approach  used  in
versions prior to 971) 
EQ.2:  Search  only  on 
the 
independent 
(unconstrained)
variables 
EQ.3:  Use adaptive line search  
EQ.4:  Use curved line search  
IRAD 
Normalized  curvature  factor  for  curved  line  search,  where  0
indicates  a  straight  line  search  and  1  indicates  full  curved  line 
search. 
SRAD 
Radius  of  influence  for  determining  curve  in  curved  line  search.
VARIABLE   
DESCRIPTION
For each independent node, all nodes within this radius are used
for  determining  the  curve.    If  0,  then  all  nodes  connected  to  the
same element as the independent node are used. 
AWGT 
SRED 
Adaptive line search weight factor between 0 and 1.  A high value
tends  to  restrict  the  motion  of  oscillating  nodes  during  the
implicit process. 
Initial  step  reduction  between  0  and  1  for  adaptive  line  search,
use large number for conservative start in implicit procedure. 
Remarks: 
  VARIABLE   
NSOLVR 
ILIMIT 
REMARKS
If  a  linear  analysis  is  selected,  equilibrium  checking  and
iterations are not performed. 
The Full Newton nonlinear solution method can be invoked by
using the default BFGS solver, and selecting ILIMIT = 1 to form 
a new stiffness matrix every iteration. 
In the neighborhood of limit points the Newton based iteration
schemes  often  fail.    The  arc  length  method  of  Riks  and
Wempner  (combined  here  with  the  BFGS  method)  adds  a 
constraint  equation  to  limit  the  load  step  to  a  constant  "arc
length"  in  load-displacement  space.    This  method  is  frequently
used to solve snap through buckling problems.  When applying 
the  arc-length  method,  the  curves  that  define  the  loading 
should contain only two points, and the first point should be at
the  origin  (0,0).    LS-DYNA  will  extrapolate,  if  necessary,  to 
determine the load.  In this  way, time and load magnitude are
related  by  a  constant.    It  is  possible  that  time  can  become
negative in case of load reversal.  The arc length method cannot
be used in a dynamic analysis. 
In  the  default  BFGS  method,  the global  stiffness  matrix  is  only
reformed  every  ILIMIT  iterations.    Otherwise,  an  inexpensive 
stiffness  update  is  applied.    By  setting  ILIMIT = 1,  a  stiffness 
reformation is performed every iteration.  This is equivalent to
the  Full  Newton  method  (with  line  search).    A  higher  value  of
ILIMIT  (20-25)  can  reduce  the  number  of  stiffness  matrix
reformations and factorizations which may lead to a significant 
reduction  in  cost.    Note  that  the  storage  requirements  for
VARIABLE   
REMARKS
MAXREF 
DCTOL 
ECTOL 
RCTOL 
DMTOL, etc. 
implicit include storing 2 vectors per iteration.  Large values of
ILIMIT will cause substantial increase in storage requirements. 
The  nonlinear  equilibrium  search  will  continue  until  the 
stiffness matrix has been reformed |MAXREF| times, with ILIMIT 
iterations  between  each  reformation.    If  equilibrium  has  not
been  found  and  MAXREF > 0,  control  will  be  passed  to  the 
automatic time step controller if it is activated.  If the automatic 
time  step  controller  is  not  active  error  termination  will  result.
When the auto time step controller is active, it is often efficient
to  choose  MAXREF = 5  and  try  another  stepsize  quickly,  rather 
than wasting too many iterations on a difficult step.  
When MAXREF < 0 and |MAXREF| matrix reformations have 
occurred convergence for the current time step is declared, with
a warning, and the simulation moves to the next time step.  This
option  should  be  used  with  caution  as  the  results  for  that 
particular time step may be wrong. 
When  the  displacement  norm  ratio  is  reduced  below  DCTOL, 
this  condition  is  satisfied.    Smaller  numbers  lead  to  more
accurate determination of equilibrium and, on the negative side,
result  in  more  iterations  and  higher  costs.    Use  NLPRINT  to 
display norm data each iteration. 
When  the  energy  norm  ratio  is  reduced  below  ECTOL,  this 
condition  is  satisfied.    Smaller  numbers  lead  to  more  strict
determination of equilibrium and, on the negative side, result in 
more  iterations  and  higher  costs.    Use  NLPRINT  to  display
norm data each iteration. 
When  the  residual  norm  ratio  is  reduced  below  RCTOL,  this 
condition  is  satisfied.    Smaller  numbers  lead  to  more  strict
determination of equilibrium and, on the negative side, result in 
more  iterations  and  higher  costs.    By  default  this  convergence
criterion  is  effectively  disabled  using  RCTOL = 1.e10.    Use 
NLPRINT to display norm data each iteration. 
For  all  nonzero  values  of  the  strict  tolerance  parameters  in 
optional  card  2b,  the  associated  criterion  must  be  satisfied  in 
addition  to  the  ones  defined  through  DCTOL,  ECTOL  and
RCTOL.  These criteria are based on the maximum norm, which
is  regarded  as  stronger  than  the  Euclidian  norm  used  for  the
other  parameters,  and  using  them  will  likely  result  in  higher
VARIABLE   
REMARKS
accuracy  at  the  price  of  more  iterations.    For  NLPRINT.GE.2  a
table  is  listed  in  the  message  and  d3hsp  for  each  iteration,
providing  the  values  associated  with  all  the  criteria  activated.
The  first  three  (DMTOL,  EMTOL  and  RMTOL)  of  these  extra
parameters  are  unitless  and  honor  the  meaning  of  both
DNORM  and  NLNORM.    The  last  four  (NTTOL,  NRTOL,
RTTOL and RRTOL) are to be given in units force, torque, force
and  torque,  respectively,  and  the  values  used  should  account 
for  the  representative  loads  in  the  problem  as  well  as  the
discretization size.  
A  line  search  is  performed  on  stiffening  systems  to  guard
against  divergence  of  Newton-based  nonlinear  solvers.    With 
the  Full  Newton  method,  it  is  sometimes  helpful  to  define  a 
large value (LSTOL = 9999.0) to effectively disable line search. 
When  computing  the  displacement  ratio,  the  norm  of  the
incremental  displacement  vector  is  divided  by  the  norm  of
“total”  displacement.    This  “total”  displacement  may  be  either
the  total  over  the  current  step,  or  the  total  over  the  entire
simulation.  The latter tends to be more lax, and can be poor at
the end of simulations where large motions develop.  For these
is  DNORM = 1,  and 
problems,  an  effective  combination 
DCTOL = 0.01 or larger. 
By  default,  a  new  stiffness  matrix  is  formed  whenever
divergence (growing out-of-balance force) is detected.  This flag 
can be used to suppress this stiffness reformation. 
By default, a new stiffness matrix is formed at the start of every
time  step.    Suppressing  this  stiffness  reformation  can  decrease
the  cost  of  simulations  which  have  many  tiny  steps  that  are
mostly linear, such as transient dynamics. 
This  flag  controls  printing  of  displacement  and  energy
convergence measures during the nonlinear equilibrium search.
If  convergence  difficulty  occurs,  this  information  is  helpful  in 
determining the problem. 
By  default,  only  translational  degrees  of  freedom  are  used  in
evaluating  convergence  norms.    Use  this  flag  to  include
rotational  degrees  of  freedom,  or  to  make  additional  data
available for diagnosing convergence problems.  
LSTOL 
DNORM 
DIVERGE 
ISTIF 
NLPRINT 
NLNORM
VARIABLE   
REMARKS
This  additional  data  includes  the  worst  offending  node  and
degree  of  freedom  contributing  to  each  norm.    Rotational
degrees  of  freedom  can  be  considered  independently  from  the
translational  degrees  of  freedom,  meaning  that  two  separate 
scalar  products  are  used  for  evaluating  norms,    〈𝐮, 𝐯〉t = 𝐮T𝐉t𝐯
and  〈𝐮, 𝐯〉r = 𝐮T𝐉r𝐯.    Here  𝐉t  and  𝐉r  are  diagonal  matrices  with 
ones  on  the  diagonal  to  extract  the  translational  and  rotational
degrees  of 
the  option
NLNORM = 1,  and  the  convergence  criteria  must  be  satisfied
for  both  translational  and  rotational  degrees  of  freedom 
simultaneously. 
freedom,  respectively. 
  This 
is 
Alternatively they can be included by defining the single scalar
product 〈𝐮, 𝐯〉 = 〈𝐮, 𝐯〉t + 𝜆𝑢𝜆𝑣〈𝐮, 𝐯〉r, where 𝜆𝑢 and 𝜆𝑣 are scale 
factors to account for different units of the rotational degrees of
freedom.    For  NLNORM = 4  these  scale  factors  are  equal  to  1, 
but  for  NLNORM < 0  𝜆𝑢  is  equal  to  |NLNORM|  if    u  is  a 
displacement vector and |NLNORM|−1 if it is a force vector, and 
the  same  goes  for  the  pair  𝜆𝑣  and  𝐯.    So  |NLNORM|  is  a 
characteristic length that appropriately weighs translational and 
rotational degrees of freedom together.  
The  arc  length  method  can  be  controlled  based  on  the
displacement  of  a  single  node  in  the  model.    For  example,  in
dome reversal problems the node at the center of the dome can
be used.  By default, the generalized arc length method is used, 
where  the  norm  of  the  global  displacement  vector  controls  the
solution.  This includes all nodes. 
In many cases the arc length method has difficulty tracking the
load  displacement  curve  through  critical  regions. 
  Using
0 < ARCLEN < 1 will reduce the step size to assist tracking the
  Use  of
load-displacement  curve  with  more  accuracy. 
ARCLEN < 1  will  cause  more  steps  to  be  taken.    Suggested
values are 1.0 (the default), 0.5, 0.25, and 0.10. 
Some  static  problems  exhibit  oscillatory  response  near
instability  points.    This  option  numerically  suppresses  these
oscillations, and may improve the convergence behavior of the
post-buckling solution. 
ARCCTL 
ARCLEN 
ARCDMP 
LMSTD 
The  default  method  for  determining  convergence  of  the 
nonlinear line search is to find the minimum of the energy.  This
VARIABLE   
REMARKS
LSDIR 
IRAD / SRAD 
parameter allows choosing the energy on only the translational
variables,  energy  of  both  the  translational  and  rotational
variables, or for minimizing the residual (forces).  The effect of 
using  a  residual  based  line  search  is  not  always  positive,
sometimes it is too restrictive and stops convergence.  However,
it is a more conservative approach than using the energy based
method  since  it  explicitly  controls  the  norm  of  the  residual.    It 
should not be seen as a better strategy than the energy method
but  as  an  alternative  to  try  in  cases  when  the  default  method
seems  to  be  working poorly.    Line  search methods  5  and  6  are
conservative  line  search  methods  to  be  used  for  highly 
nonlinear problems, these should not be used as default but as
final resorts to potentially resolve convergence issues.  The rule
of  thumb  is  that  the  LSMTD = 5  is  slow  but  robust  and 
LSMTD = 6 is even slower but more robust. 
In  Version  971  of  LS-DYNA  new  line  search  options  were 
added.  The traditional approach (LSDIR = 1) computes the line 
search direction using all variables.  The new (default) approach
of  LSIDR = 2  computes  the  line  search  direction  only  on  the
unconstrained  variables.    It  has  proven  to  be  both  robust  and 
more  efficient.    We  have  also  included  two new  approaches  to
try for problems where the default and traditional approach fail
and  the  user  is  using  Full  Newton  (ILIMIT = 1).    See  the  next 
two remarks for more information on those methods. 
The parameters IRAD and SRAD are for the curved line search
(LSDIR = 4).    The  first  parameter  is  a  switch  (0  or  1)  to  invoke
this  line  search,  an  intermediate  value  is  interpreted  as
weighted combination of a straight and curved line search (the 
curvature  radius  is  decreased  with  increasing  IRAD).    A  value
of  unit  is  recommended  in  situations  with  rather  smooth
responses,  e.g.    springback  and  similar  problems.    Also,
IRAD = 1 seems to work best with full Newton iterations.  The 
SRAD  parameter  should  be  equal  to  0  for  most  cases,  this
means that the search curve for a node is determined from the
search  direction  of  nodes  connected  to  the  same  elements  as
that node.  SRAD > 0 is interpreted as a radius of influence,  
meaning  that  the  search  curve  for  a  node  is  determined  from
the  search  direction  of  nodes  within  a  distance  SRAD  of  this
node.    This  option  was  introduced  as  an  experiment  to  see  if
this  had  a  smoothing  and  stabilizing  effect.    A  value  of  0.0  is
VARIABLE   
REMARKS
currently recommended. 
AWGT / SRED 
The  parameters  AWGT  and  SRED  are  for  the  adaptive  line
search.    The  intention  is  to  improve  robustness  for  problems
that  have  tendencies  to  oscillate  or  diverge,  indicated  by  the
dnorm and enorm parameter outputs in the iterations (stdout). 
A  value  of  0.5  is  recommended  for  AWGT  as  a  starting  point.
With  a  nonzero  value  the  motions  of  individual  nodes  are
tracked.  For nodes that are oscillating (going back and forth in
space), the maximum step size for the next iteration is reduced
in  proportion  to  the  parameter  AWGT,  and  for  nodes  that  are
not  oscillating  but  going    nicely  along  a  straight  path,  the
maximum  step  size  for  the  next  iteration  is  increased  in
proportion to 1-AWGT. 
In  test  problems,  the  introduction  of  the  adaptive  line  search 
has  stabilized  the  implicit  procedure  in  the  sense  that  the
dnorm  and  enorm  values  are  more  monotonically  decreasing
until convergence with virtually no oscillations.  If a problem is
still oscillating or diverging, the user should try to increase the 
AWGT  parameter  since  this  is  a  more  restrictive  approach  but
probably gives a slower convergence rate.  An option for nasty
problems  is  also  to  use  SRED > 0  which  is  the  initial  step 
reduction  factor  (less  than  1).    This  means  that  the  initial  step
size  is  reduced  by  this  value  but  the  maximum  step  size  will
increase by an amount that is determined by the success in the
iterative procedure, eventually it will reach unity.  It can never
decrease.  Also here, it is intended to be used with full Newton
method.
*CONTROL_IMPLICIT_SOLVER_{OPTION} 
Available options include: 
<BLANK> 
DYN 
SPR 
Purpose:  These optional cards apply to implicit calculations.  The linear equation solver 
performs  the  CPU-intensive  stiffness  matrix  inversion  .    The  DYN  option  allows  setting  controls  specifically  for  the  dynamic 
relaxation phase.  The SPR option allows setting controls specifically for the springback 
phase. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LSOLVR 
LPRINT 
NEGEV 
ORDER 
DRCM 
DRCPRM  AUTOSPC  AUTOTOL
Type 
I 
Default 
4 
I 
0 
I 
2 
I 
0 
I 
4 
F 
see 
below 
I 
1 
F 
see 
below 
Card 2 is optional. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCPACK  MTXDMP 
Type 
Default 
I 
2 
I
VARIABLE   
DESCRIPTION
LSOLVR 
Linear equation solver method . 
EQ.4:  SMP parallel multi-frontal sparse solver (default). 
EQ.5:  SMP  parallel  multi-frontal  sparse  solver,  double 
precision 
EQ.6:  BCSLIB-EXT, direct, sparse, double precision 
EQ.10:  iterative, best of currently available iterative methods 
EQ.11:  iterative, Conjugate Gradient method 
EQ.12:  iterative, CG with Jacobi preconditioner 
EQ.13:  iterative, CG with Incomplete Choleski preconditioner 
EQ.14:  iterative, Lanczos method 
EQ.15:  iterative, Lanczos with Jacobi preconditioner 
EQ.16:  iterative,  Lanczos  with  Incomplete  Choleski  precondi-
tioner 
LPRINT 
Linear  solver  print  flag  controls  screen  and  message  file  output
. 
EQ.0: no printing 
EQ.1: output summary statistics on memory, cpu requirements
EQ.2: more statistics 
EQ.3: even more statistics and debug checking 
NOTE:  during execution, use the interactive command "<ctrl-
c> lprint" to toggle this print flag between 0 and 1. 
NEGEV 
Negative  eigenvalue  flag.    Selects  procedure  when  negative
eigenvalues  are  detected  during  stiffness  matrix  inversion  . 
EQ.1: stop, or retry step if auto step control is active 
EQ.2: print warning message, try to continue (default) 
ORDER 
Ordering option  
EQ.0: method set automatically by LS-DYNA 
EQ.1: MMD, Multiple Minimum Degree. 
EQ.2: Metis
VARIABLE   
DRCM 
DESCRIPTION
Drilling  rotation  constraint  method  for  shells  . 
EQ.1: add drilling stiffness (old Version 970 method) 
DRCPRM 
EQ.2: same as 4 below 
EQ.3: add no drilling stiffness 
EQ.4: add drilling stiffness  (improved method) (default) 
Drilling  rotation  constraint  parameter  for  shells.    This  parameter
scales  the  drilling  stiffness.    For  the  old  method  (DRCM = 1)  the 
default  value  of  DRCPRM  is  1.0  for  linear  analysis,  100.0  for 
nonlinear  implicit  analysis,;  and  either  1.E-12  or  1.E-8  for 
eigenvalue  analysis  depending  on  the  shell  element  type.    For
eigenvalue analysis, the input value for DRCPRM is ignored.  For
the  improved  method  (default,  DRCM = 4),  the  default  value  of 
DRCPRM is as described above for the old method except default
DRCPRM is 1.0  for nonlinear implicit analysis. 
AUTOSPC 
Automatic Constraint Scan flag 
EQ.1: scan 
the  assembled  stiffness  matrix 
for
unconstrained, unattached degrees of freedom.  Generate 
additional  constraints  as  necessary  to  avoid  negative
eigenvalues. 
looking 
EQ.2: do not add constraints. 
AUTOTOL 
AUTOSPC  tolerance.    The  test  for  singularity  is  the  ratio  of  the
smallest singular value and the largest singular value.  If this ratio
is  less  than  AUTOTOL,  then  the  triple  of  columns  are  declared
singular  and  a  constraint  is  generated.    Default  value  in  single 
precision is 10−4 and in double precision, 10−8. 
LCPACK 
Matrix assembly package. 
MTXDMP 
EQ.2: Use  v970’s  LCPACK  (default,  only  available  option  in
971) 
EQ.3:  Same  as  2,  but  incorporates  a  non-symmetric  linear 
solver, see remark for LCPACK. 
Matrix  and  right-hand-side  dumping.    LS-DYNA  has  the  option 
of  dumping  the  globally  assembled  stiffness  matrix  and  right-
hand-side  vectors  files  in  Harwell-Boeing  sparse  matrix  format. 
Such output may be useful for comparing to other linear equation
solution packages.
VARIABLE   
DESCRIPTION
EQ.0: No dumping 
GT.0:  Dump  all  matrices  and  right-hand-side  vectors  every 
MTXDMP  time  steps.    Output  is  written  as  ASCII  text
and the iinvolved filenames are of the following form: 
K_xxxx_yyy.mtx.rb 
This file contains the stiffness matrix at step xxxx, it-
eration yyy. 
M_xxxx_yyy.mtx.rb 
This file contains the mass matrix at step xxxx, itera-
tion.  Only for eigenvalue analysis.  
MW_xxxx_yyy.mtx.rb 
This file contains the damping matrix at step xxxx, it-
eration.  Only for simulations with damping. 
K_xxxx_yyy_zzz.rhs.rb 
This file contains the right hand side at step xxxx, it-
eration  yyy,  where  yyy  is  the  iteration  at  which  a 
stiffness matrix is formed; zzz is the cumulative itera-
tion number for the step.  The values of yyy and zzz
don’t always coincide  because the stiffness matrix is
not necessarily reformed every iteration. 
Node_Data_xxxx_yyy 
This file maps stiffness matrix to nodes and provides
nodal coordinates. 
LT.0: 
Like positive values of MTXDMP but dumped data
is binary. 
EQ.|9999|:  Simulation  is  terminated  after  dumping  matrices
and right hand side prior to factorization. 
Remarks: 
  VARIABLE   
LSOLVR 
REMARKS
The  linear  solver  is  used  to  compute  the  inverse  of  the  global
stiffness matrix, which is a costly procedure both in memory and
cpu  time.    Direct  solvers  apply  Gaussian  elimination,  while
iterative  solvers  successively  improve  “guesses”  at  the  correct
solution.    Iterative  solvers  require  far  less  memory  than  direct
VARIABLE   
REMARKS
solvers,  but  may  suffer  from  convergence  problems.    Generally,
iterative solvers are poor for automotive applications, but can be
superior for large brick element soil models in civil engineering. 
Solvers  5  and  6  promote  the  global  matrix  to  double  precision
before  factoring  to  reduce  numerical  truncation  error.    Solvers  4
and 5 are equivalent if a double precision executable is used. 
Solver  6  is  the  direct  linear  equation  solver  from  BCSLIB-EXT, 
Boeing's  Extreme  Mathematical  Library.    This  option  should  be
used whenever the factorization is too large to fit into memory.  It
has  extensive  capabilities  for  out-of-core  solution  and  can  solve 
larger  problems  than  any  of  the  other  direct  factorization
methods.  Solver 6 also includes a sophisticated pivoting strategy
which can be superior for nearly singular matrices. 
Solver 5 is the only option supported in MPP. 
LPRINT 
NEGEV 
the 
storage 
timing  and 
Select  printing  of 
information
(LPRINT = 1)  if  you  are  comparing  performance  of  linear 
equation  solvers,  or  if  you  are  running  out  of  memory  for  large
models.  Minimum memory requirements for in-core and out-of-
core  solution  are  printed.    This  flag  can  also  be  toggled  using
sense  switch  "<ctrl-c>  lprint".    For  best  performance,  increase 
available memory using “memory=“ on the command line until an IN-
CORE solution is indicated. 
When  using  solver  option  6,  LPRINT = 2  and  3  will  cause 
increased  printed  output  of 
statistics  and  performance
information. 
Negative eigenvalues result from underconstrained models (rigid
body  modes),  severely  deformed  elements,  or  non-physical 
material properties.  This flag allows control to be passed directly
to  the  automatic  time  step  controller  when  negative  eigenvalues
are  detected.    Otherwise,  significant  numerical  roundoff  error  is
likely  to  occur  during  factorization,  and  equilibrium  iterations
may fail .
ORDER 
DRCPRM 
LCPACK 
*CONTROL_IMPLICIT_SOLVER 
REMARKS
The  system  of  linear  equations  is  reordered  to  optimize  the
sparsity of the factorization when using direct methods.  Metis is
a  ordering  method  from  University  of  Minnesota  which  is  very
effective for larger problems and for 3D solid problems, but also
very  expensive.    MMD  is  inexpensive,  but  may  not  produce  an
optimum  reordering,  leading  to  higher  cost  during  numeric 
factorization.    MMD  is  usually  best  for  smaller  problems  (less
than 100,000 degrees of freedom). 
Reordering cost is included in the symbolic factorization phase of
the  linear  solver  (LSPRINT ≥ 1).    For  large  models,  if  this  cost 
exceeds  20%  of  the  numeric  factorization  cost,  it  may  be  more
efficient to select the MMD method. 
Note  that  the  values  of  LPRINT  and  ORDER  also  affect  the
eigensolution  software.    That  is  LPRINT  and  ORDER  from  this
keyword card is applicable to eigensolution. 
To  avoid  a  singular  stiffness  matrix  in  implicit  analysis  of  flat
shell  topologies,  some  constraint  on  the  drilling  degree  of
freedom  is  needed.      The  default  method  of  applying  this
constraint,  DRCPRM = 4,  adds  the  consistent  force  vector  for 
consistency  and  improved  convergence  as  compared  to  the  old
method, DRCPRM = 1. 
In  explicit  analysis,  an  unconstrained  drilling  degree  of  freedom
is  usually  not  a  concern  since  a  stiffness  matrix  is  not  used.
However, special situations may arise in which the user wishes to 
include additional resisting rotational force in the drilling degree
of freedom for improved robustness and/or accuracy.  To activate
the consistent drilling constraint in explicit analysis, use the input
variables DRCPSID and DRCPRM for *CONTROL_SHELL. 
Certain features may break the symmetry of the stiffness matrix.
Unless LCPACK is set to 3 these contributions are suppressed or
symmetrized  by  the  default  symmetric  linear  solver.    However,
when LCPACK is set to 3 a more general linear solver lifting the 
symmetry  requirement  is  used.    The  solver  for  non-symmetric 
matrices is more computationally expensive. 
Keywords 
implemented are listed below: 
for  which 
the  non-symmetric  contribution 
is 
*CONTACT_..._MORTAR:
VARIABLE   
REMARKS
The  mortar  contact  accounts  for  frictional  non-symmetry 
in  the  resulting  tangent  stiffness  matrix,  the  effects  on
convergence  characteristics  have  not  yet  shown  to  be
significant. 
*LOAD_SEGMENT_NONUNIFORM: 
The non-symmetric contribution may be significant for the
follower load option, LCID < 0. 
*LOAD_SEGMENT_SET_NONUNIFORM: 
The non-symmetric contribution may be significant for the
follower load option, LCID < 0. 
*MAT_FABRIC_MAP: 
This  stress  map  fabric  model  accounts  for  non-symmetry 
in  the  material  tangent  modulus,  representing  the  non-
linear Poisson effect due to complex interaction of yarns.   
*SECTION_SHELL, *SECTION_SOLID: 
User defined resultant elements (ELFORM = 101, 102, 103, 
104, 105 with NIP=0) support the assembly and solution of 
non-symmetric element matrices. 
*SECTION_BEAM: 
Belytschko-Schwer  beam 
geometric stiffness contribution is supported. 
(ELFORM=2)  nonsymmetric
*CONTROL_IMPLICIT_STABILIZATION_{OPTION} 
Available options include: 
<BLANK> 
DYN 
SPR 
Purpose:    This  optional  card  applies  to  implicit  calculations.    Artificial  stabilization  is 
required  for  multi-step  unloading  in  implicit  springback  analysis  .  The DYN option allows setting controls specifically for 
the  dynamic  relaxation  phase.    The  SPR  option  allows  setting  controls  specifically  for 
the springback phase. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IAS 
SCALE 
TSTART 
TEND 
Type 
I 
F 
F 
F 
Default 
2 
1.0 
see 
below 
see 
below 
  VARIABLE   
DESCRIPTION
IAS 
Artificial Stabilization flag 
EQ.1: active 
EQ.2: inactive (default) 
SCALE 
Scale factor for artificial stabilization.  For flexible parts with large
springback,  like  outer  body  panels,  a  value  of  0.001  may  be
required. 
EQ.-n: curve ID = n gives SCALE as a function of time 
TSTART 
Start time.  (Default:  immediately upon entering implicit mode) 
TEND 
End time.  (Default: termination time)
Remarks: 
Artificial  stabilization  allows  springback  to  occur  over  several  steps.    This  is  often 
necessary  to  obtain  convergence  during  equilibrium  iterations  on  problems  with  large 
springback  deformation.    Stabilization  is  introduced  at  the  start  time  TSTART,  and 
slowly  removed  as  the  end  time  TEND  is  approached.    Intermediate  results  are  not 
accurate  representations  of  the  fully  unloaded  state.    The  end  time  TEND  must  be 
reached exactly for total springback to be predicted accurately. 
  VARIABLE   
IAS 
SCALE 
REMARKS 
The default for IAS depends on the analysis type in *CONTROL_-
IMPLICIT_GENERAL. 
  For  “seamless”  springback  analysis,
automatic  time  step  control  and  artificial  stabilization  are
activated by default.  Otherwise, IAS is inactive by default. 
This  is  a  penalty  scale  factor  similar  to  that  used  in  contact
interfaces.    If  modified,  it  should  be  changed  in  order-of-
magnitude increments at first.  Large values suppress springback
deformation  until  very  near  the  termination  time,  making
convergence  during  the  first  few  steps  easy.    Small  values  may
not  stabilize  the  solution  enough  to  allow  equilibrium  iterations
to converge.
*CONTROL_IMPLICIT_STATIC_CONDENSATION_{OPTION} 
Available options include: 
<BLANK> 
BINARY 
Purpose:  Request static condensation of a part to build a reduced linearized model for 
later  computation  with  *ELEMENT_DIRECT_MATRIX_INPUT. 
  Optionally  the 
analysis can continue using the linearization for the current analysis. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  SC_FLAG  SC_NSID  SC_PSID  SE_MASS SE_STIFF SE_INERT 
I 
0 
2 
I 
0 
3 
Type 
Default 
I 
0 
  Card 2 
1 
Variable 
Type 
C 
C 
C 
4 
5 
6 
7 
8 
SE_FILENAME 
A80 
  VARIABLE 
DESCRIPTION
SC_FLAG 
Static Condensation Control Flag 
EQ.0: no static condensation will be performed  
EQ.1: create  superelement  representation  based  on  static
condensation. 
EQ.2: use static condensation to build a linearized representa-
tion  for  a  part  and  use  that  linearized  representation  in
the following analysis. 
SC_NSID 
Node set ID for nodes to be preserved in the static condensation
procedure.  Required when SC_FLAG = 1.
VARIABLE 
SC_PSID 
SE_MASS 
SE_STIFF 
SE_INERT 
DESCRIPTION
Part  set  ID  for  parts  to  be  included  in  the  static  condensation 
procedure.  When SC_FLAG = 1, SC_PSID can be used to specify 
a  subset  of  the  model  with  the  default  being  the  entire  model.
When  SC_FLAG = 2,  SC_PSID  is  required.    SC_PSID = 0  implies 
that the entire model is condensed. 
Name  of  the  superelement  mass  matrix.    If  left  blank  it  is  not
generated. 
Name of the superelement stiffness matrix.  If left blank it is not
generated. 
Name  of  the  superelement  inertia  matrix,  required  for  gravity
loading  applications  of  the  superelement.    If  left  blank  it  is  not
generated. 
SE_FILENAME 
If  any  of  SE_MASS,  SE_STIFF,  or  SE_INERT  is  blank  then  the 
second  line  is  required  and  contains  the  file  name  for  the
superelement. 
Remarks: 
To use this feature, an implicit analysis must be requested using IMFLAG = 1 on *CON-
TROL_IMPLICIT_GENERAL,  and  a  non-zero  termination  time  must  be  specified  on 
*CONTROL_TERMINATION.  A double precision version of LS-DYNA should be used 
for best accuracy.  The superelement model is written to file SE_FILENAME.   
Static  condenstation  is  the  reduction  of  the  global  stiffness  and  mass  matrices  to  a 
specified sets of rows and columns associated with the nodes in the node set SC_NSID.  
The first and second node set attribute parameters can be optionally used to restrict the 
translational  and  rotational  degrees  of  freedom  for  which  modes  are  requested, 
respectively, according to the following syntax: 
Node set attribute parameters DA1 and A1:  translational degree of freedom codes 
Node set attribute parameters DA2 and A2:  rotational degree of freedom codes
Code 
0 
1 
2 
3 
4 
5 
6 
7 
Modes Computed 
 
X degree of freedom only 
Y degree of freedom only 
Z degree of freedom only 
X, Y degrees of freedom only 
Y, Z degrees of freedom only 
X, Z degrees of freedom only 
X, Y, Z degrees of freedom 
Setting both node set attributes to zero is equivalent to setting both node set attributes 
to 7 (X, Y, and Z for translational and rotational degrees of freedom). 
If one node set attribute is nonzero (codes 1 to 7) and the other node set attribute is zero, 
then the zero attribute means  NO degrees of freedom are considered.  For example, if 
DA1 = 2  and  DA2 = 0,  then  only  the  Y-translational  degree  of  freedom  modes  are 
calculated. 
The user can create the superelement representation of the reduced model by specifying 
the  SE_MASS,  SE_STIFF,  SE_INERT  and  SE_FILENAME  fields.    This  implementation 
does  not  include  SE_DAMP.    The  file,  by  default  is  written  in  the  Nastran  DMIG  file 
format  and  can  be  used  as  input  to  *ELEMENT_DIRECT_MATRIX_INPUT.    The 
keyword  option  BINARY  can  be  used  to  create  a  binary  representation  for  the 
superelement which can be used with *ELEMENT_DIRECT_MATRIX_INPUT_BINARY 
to reduce the file size. 
Static Condensation is equivalent to using only constraint modes with *CONTROL_IM-
PLICIT_MODES.    Static  Condensation  does  have  the  ability  to  continue  the  analysis 
using the linear representation for a part set.
*CONTROL_IMPLICIT_TERMINATION 
Purpose:  Specify termination criteria for implicit transient simulations. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DELTAU 
DELTA1 
KETOL 
IETOL 
TETOL 
NSTEP 
Type 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
I 
3 
  VARIABLE   
DELTAU 
DESCRIPTION
Terminate  based  on  relative  total  displacement  in  the  Euclidean
norm. 
GT.0.0: terminate  when  displacement  in  the  Euclidean  norm 
for  last  time  step  relative  to  the  total  displacement  in
the Euclidean norm is less than DELTAU. 
DELTA1 
Terminate based on relative total displacement in the max norm. 
GT.0.0: terminate when displacement in the max norm for last
time  step  relative  to  the  total  displacement  in  the  max 
norm is less than DELTAU. 
KETOL 
Terminate based on kinetic energy 
GT.0.0: terminate when kinetic energy drops below KETOL for
NSTEP consecutive implicit time steps. 
IETOL 
Terminate based on internal energy 
GT.0.0: terminate when internal energy drops below IETOL for
NSTEP consecutive implicit time steps. 
TETOL 
Terminate based on total energy 
GT.0.0: terminate  when  total  energy  drops  below  TETOL  for
NSTEP consecutive implicit time steps. 
NSTEP 
Number  of  steps  used  in  the  early  termination  tests  for  kinetic,
internal, and total energy.
*CONTROL_IMPLICIT_TERMINATION 
For  some  implicit  applications  it  is  useful  to  terminate  when  there  is  no  change  in 
displacement  or  low  energy.    This  keyword  provides  the  ability  to  specify  such  a 
stopping criterias to terminate the simulation prior to ENDTIM.
*CONTROL 
Purpose:  Define global control parameters for material model related properties. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MAEF 
Type 
Default 
I 
0 
  VARIABLE   
DESCRIPTION
MAEF 
Failure options:  
EQ.0: all *MAT_ADD_EROSION definitions are active. 
EQ.1: switch  off  all 
*MAT_ADD_EROSION  definitions 
globally.    This  feature  is  useful  for  larger  models  where
removing  the  *MAT_ADD_EROSION  cards  is  incon-
vient.
*CONTROL_MPP 
Purpose:  Set control parameters for MPP specific features. 
*CONTROL_MPP_CONTACT_GROUPABLE 
*CONTROL_MPP_DECOMPOSITION_ARRANGE_PARTS 
*CONTROL_MPP_DECOMPOSITION_AUTOMATIC 
*CONTROL_MPP_DECOMPOSITION_BAGREF 
*CONTROL_MPP_DECOMPOSITION_CHECK_SPEED 
*CONTROL_MPP_DECOMPOSITION_CONTACT_DISTRIBUTE 
*CONTROL_MPP_DECOMPOSITION_CONTACT_ISOLATE 
*CONTROL_MPP_DECOMPOSITION_DISABLE_UNREF_CURVES 
*CONTROL_MPP_DECOMPOSITION_DISTRIBUTE_ALE_ELEMENTS 
*CONTROL_MPP_DECOMPOSITION_DISTRIBUTE_SALE_ELEMENTS 
*CONTROL_MPP_DECOMPOSITION_DISTRIBUTE_SPH_ELEMENTS 
*CONTROL_MPP_DECOMPOSITION_ELCOST 
*CONTROL_MPP_DECOMPOSITION_FILE 
*CONTROL_MPP_DECOMPOSITION_METHOD 
*CONTROL_MPP_DECOMPOSITION_NUMPROC 
*CONTROL_MPP_DECOMPOSITION_OUTDECOMP 
*CONTROL_MPP_DECOMPOSITION_PARTS_DISTRIBUTE 
*CONTROL_MPP_DECOMPOSITION_PARTSET_DISTRIBUTE 
*CONTROL_MPP_DECOMPOSITION_RCBLOG 
*CONTROL_MPP_DECOMPOSITION_SCALE_CONTACT_COST 
*CONTROL_MPP_DECOMPOSITION_SCALE_FACTOR_SPH 
*CONTROL_MPP_DECOMPOSITION_SHOW
*CONTROL_MPP_DECOMPOSITION_TRANSFORMATION 
*CONTROL_MPP_IO_LSTC_REDUCE 
*CONTROL_MPP_IO_NOBEAMOUT 
*CONTROL_MPP_IO_NOD3DUMP 
*CONTROL_MPP_IO_NODUMP 
*CONTROL_MPP_IO_NOFAIL 
*CONTROL_MPP_IO_NOFULL 
*CONTROL_MPP_IO_SWAPBYTES 
*CONTROL_MPP_MATERIAL_MODEL_DRIVER 
*CONTROL_MPP_PFILE
*CONTROL_MPP_CONTACT_GROUPABLE 
Purpose:    Allow  for  global  specification  that  the  GROUPABLE  algorithm  should  be 
enabled/disabled for contacts when running MPP. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
GRP 
Type 
I 
Default 
none 
  VARIABLE   
GRP 
DESCRIPTION
The  sum  of  these  available  options  (in  any  combination  that
makes sense): 
1:  Turn on GROUPABLE for all non-tied contacts 
2:   Turn on GROUPABLE for all tied contacts 
4:   Turn off GROUPABLE for all non-tied contacts 
8:   Turn off GROUPABLE for all tied contacts 
Remarks: 
The  GROUPABLE  algorithm  is  an  alternate  MPP  communication  algorithm  for  SIN-
GLE_SURFACE,  NODE_TO_SURFACE,  and  SURFACE_TO_SURFACE  contacts.    This 
algorithm does not support all contact options, including SOFT = 2, as of yet, and is still 
under  development.    It  can  be  significantly  faster  and  scale  better  than  the  normal 
algorithm when there are more than two or three applicable contact types defined in the 
model.  Its intent is to speed up the contact processing but not to change the behavior of 
the contact. 
 This  keyword  will  override  any  setting  of  the  GRPABLE  parameter  on  the  *CON-
TACT_…_MPP card, and is intended as a way to quickly experiment with this feature.  
The equivalent pfile option is “contact { groupable GRP }” where GRP is an integer as 
described above.
*CONTROL_MPP_DECOMPOSITION_ARRANGE_PARTS_OPTION 
Purpose:  Allow users to distribute certain part(s) to all processors or to isolate certain 
part(s) in a single processor.  This keyword supports multiple entries.  Each entry is be 
processed as a separate region for decomposition. 
When  this  keyword  is  part  of  an  included  file  and  the  LOCAL  option  is  given,  the 
decomposition will be done in the coordinate system of the included file, which may be 
different from the global system, if the file is included using the *INCLUDE_TRANS-
FORM keyword. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
TYPE 
NPROC 
FRSTP 
Type 
I 
I 
I 
I 
Default 
none 
none 
None 
None 
  VARIABLE   
DESCRIPTION
ID 
TYPE 
Part ID/Part set ID 
EQ.0:  Part ID to be distributed to all processors 
EQ.1:  Part Set ID to be distributed to all processors 
EQ.10:  Part ID to be lumped into one processor 
EQ.11:  Part Set ID to be lumped into one processor. 
NPROC 
Used  only  for  TYPE  equal  to  0  or  1.    Evenly  distributed  Part
ID/Part set ID to NPROC of processors. 
FRSTP 
Used only for TYPE equal to 0 or 1.  Starting MPP rank ID. 
Remarks: 
There is no equivalent option under pfile.
*CONTROL_MPP_DECOMPOSITION_AUTOMATIC 
Purpose:    Instructs  the  program  to  apply  a  simple  heuristic  to  try  to  determine  the 
proper decomposition for the simulation. 
There  are  no  input  parameters.    The  existence  of  this  keyword  triggers  the  automated 
decomposition.  This option should not be used if there is more than one occurrence of 
any of the following options in the model: 
*INITIAL_VELOCITY 
*CHANGE_VELOCITY 
*BOUNDARY_PRESCRIBED_MOTION 
And the following control card must not be used: 
*CONTROL_MPP_DECOMPOSITION_TRANSFORMATION 
For  the  general  case,  it  is  recommended  that  you  specify  the  proper  decomposition 
using 
*CONTROL_MPP_DECOMPOSITION_TRANSFORMATION 
instead.
the  command
*CONTROL_MPP_DECOMPOSITION_BAGREF 
Purpose:    With  this  card  LS-DYNA  performs  decomposition  according  to  the  airbag’s 
reference geometry, rather than the folded geometry. 
Other  than  BAGID  values  this  card  takes  no  input  parameters.    The  initial  geometry 
may lead to a poor decomposition once the bag is deployed.  This option will improve 
load balancing for the fully deployed geometry. 
Optional card(s) for selected reference geometry ID 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BAGID1 
BAGID2 
BAGID3 
BAGID4 
BAGID5 
BAGID6 
BAGID7 
BAGID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
BAGIDi 
DESCRIPTION
ID  defined 
*AIRBAG_SHELL_REFERENCE_GEOMETRY_ID 
in  *AIRBAG_REFERENCE_GEOMETRY_ID  or 
Bags  specified  in  the  optional  cards  will  be  decomposed  based  on  the  reference 
geometry.    If  there  is  no  card  given,  all  bags  will  be  decomposed  by  their  reference 
geometry. 
Remarks: 
Command in partition file (pfile): BAGREF. The option for selecting particular airbags is 
only available when using keyword input.
*CONTROL_MPP_DECOMPOSITION_CHECK_SPEED 
Purpose:  Modifies the decomposition depending on the relative speed of the processors 
involved. 
There  are  no  input  parameters.    Use  of  this  keyword  activates  a  short  floating  point 
timing  routine  to  be  executed  on  each  processor.    The  information  gathered  is  used 
during the decomposition, with faster processors being given a relatively larger portion 
of the problem.  This option is not recommended on homogeneous systems.
*CONTROL_MPP_DECOMPOSITION_CONTACT_DISTRIBUTE_OPTION 
Purpose:    Ensures  that  the  indicated  contact  interfaces  are  distributed  across  all 
processors,  which  can  lead  to  better  load  balance  for  large  contact  interfaces.    If  this 
appears in an included file and the LOCAL option is given, the decomposition will be 
done  in  the  coordinate  system  of  the  included  file,  which  may  be  different  from  the 
global system if the file is included via *INCLUDE_TRANSFORM. 
  Card 1 
1 
Variable 
ID1 
2 
ID2 
3 
ID3 
4 
ID4 
5 
ID5 
6 
7 
8 
Type 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
DESCRIPTION
First  contact  interface  ID  to  distribute.    If  no  contact  ID's  are
specified, the number given here corresponds to the order of the
interfaces as they appear in the input, with the first being 1. 
Remaining interfaces ID's to distribute. 
  VARIABLE   
ID1 
ID2, ID3, 
ID4, ID5 
Remarks: 
Up  to  5  contact  interface  ID's  can  be  specified.    The  decomposition  is  modified  as 
follows:    First,  all  the  elements  involved  in  the  first  contact  interface  are  decomposed 
across all the processors.  Then all the elements involved in the second contact interface 
(excluding any already assigned to processors) are distributed, and so on.  After all the 
contact interfaces given are processed, the rest of the input is decomposed in the normal 
manner.  This will result in each processor having possibly several disjoint portions of 
the input assigned to it, which will increase communications somewhat.  However, this 
can be offset by improved load balance in the contact.  It is generally recommended that 
at most one or two interfaces be specified, and then only if they are of substantial size 
relative to the whole problem.
*CONTROL_MPP_DECOMPOSITION_CONTACT_ISOLATE 
Purpose:  Ensures that the indicated contact interfaces are isolated on a single processor, 
which can lead to decreased communication. 
  Card 1 
1 
Variable 
ID1 
2 
ID2 
3 
ID3 
4 
ID4 
5 
ID5 
6 
7 
8 
Type 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
DESCRIPTION
First  contact  interface  ID  to  isolate.    If  no  contact  ID's  are
specified, the number given here corresponds to the order of the
interfaces as they appear in the input, with the first being 1. 
Remaining interfaces ID's to isolate. 
  VARIABLE   
ID1 
ID2, ID3, 
ID4, ID5 
Remarks: 
Up to 5 contact interfaces can be specified.  The decomposition is modified as follows:  
First, all the elements involved in the first contact interface ID are assigned to the first 
processor.  Then all the elements involved in the second contact interface ID (excluding 
any already assigned to processors) are assigned to the next processor, and so on.  After 
all the contact interfaces given are processed, the rest of the input is decomposed in the 
normal  manner.    This  will  result  in  each  of  the  interfaces  being  processed  on  a  single 
processor.    For  small  contact  interfaces  this  can  result  in  better  parallelism  and 
decreased communication.
Purpose:  Disable unreferenced time dependent load curves for the following keyword. 
*BOUNDARY_PRESCRIBED_MOTION_NODE 
*LOAD_NODE 
*LOAD_SHELL_ELEMENT 
*LOAD_THERMAL_VARIABLE_NODE 
The  details  of  this  operation  are  reported  in  each  processor’s  scratch  “scr####”  file.  
This will skip the curve evaluation on each cycle, and improve the parallel efficiency. 
Remarks: 
Command in partition file (pfile): DUNREFLC.
*CONTROL_MPP_DECOMPOSITION_DISTRIBUTE_ALE_ELEMENTS 
Purpose:  Ensures ALE elements are evenly distributed to all processors 
There  are  no  input  parameters  and  the  card  below  is  optional.    ALE  elements  usually 
have higher computational cost than other type of elements and it is better to distribute 
them  to  all  CPU  for  better  load  balance.    The  existence  of  this  keyword  causes 
DYNA/MPP  to  extract  ALE  parts  from  input  and  then  evenly  distributed  to  all 
processors. 
The card is optional 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  OVERLAP 
Type 
I 
Default 
none 
  VARIABLE   
OVERLAP 
DESCRIPTION
For  FSI  models  where  structures  are  inside  ALE  meshes  ,  decompose 
structure and ALE domains together instead of first the structure
and then ALE .  
Set type: 
EQ.0:  Off 
EQ.1:  On  
Remarks: 
1.  Command in partition file (pfile): ALEDIST. 
2.  Most  of  the  processors  will  have  to  deal  with  MPP  subdomains  from  the 
structure and ALE meshes: a portion of the ALE computational domain and a 
portion  of  the  structure  meshes.    The  default  decomposition  (first  divide  the 
structures,  then  ALE)  does  not  always  overlap  these  subdomains.    The  more 
they overlap, the lesser the MPP communications in the coupling cost.  Cutting 
the ALE and structure meshes together allows their MPP subdomains to be as 
inclusive as possible.
*CONTROL_MPP_DECOMPOSITION_DISTRIBUTE_SPH_ELEMENTS 
Purpose:  Ensures SPH elements are evenly distributed to all processors 
There are no input parameters.  SPH elements usually have higher computational cost 
than other type of elements and it is better to distribute them to all CPU for better load 
balance.  The existence of this keyword causes DYNA/MPP to extract SPH parts from 
input and then evenly distributed to all processors. 
Remarks: 
Command in partition file (pfile): SPHDIST.
*CONTROL_MPP_DECOMPOSITION_ELCOST 
Purpose:  Instructs the program to use a hardware specific element cost weighting for 
the decomposition 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ITYPE 
Type 
I 
Default 
none 
  VARIABLE   
DESCRIPTION
ITYPE 
Hardware specific cost profile. 
EQ.1: Fujitsu PrimePower 
EQ.2: Intel IA 64, AMD Opteron 
EQ.3: Intel Xeon 64 
EQ.4: General profile 
Remarks: 
Command in partition file (pfile): elcost itype.
*CONTROL_MPP_DECOMPOSITION_FILE 
Purpose:  Allow for pre-decomposition and a subsequent run or runs without having to 
do the decomposition. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
NAME 
A80 
none 
  VARIABLE   
DESCRIPTION
NAME 
Name of a file containing (or to contain) a decomposition record. 
Remarks: 
If  the  indicated  file  does  not  exist,  it  is  created  with  a  copy  of  the  decomposition 
information from this run.  If the file exists, it is read and the decomposition steps can 
be  skipped.    The  original  run  that  created  the  file  must  be  for  a  number  of  processors 
that  is  a  multiple  of  the  number  of  processors  currently  being  used.    Thus,  a  problem 
can be decomposed once for, say, 48 processors.  Subsequent runs are then possible on 
any number that divides 48: 1, 2, 3, 4, 6, etc.  Since the decomposition phase generally 
requires  more  memory  than  execution,  this  allows  large  models  to  be  decomposed  on 
one system and run on another (provided the systems have compatible binary formats).  
The file extension “.pre” is added automatically.
*CONTROL_MPP_DECOMPOSITION_METHOD 
Purpose:  Specify the decomposition method to use. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
  VARIABLE   
NAME 
NAME 
A80 
RCB 
DESCRIPTION
Name  of  the  decomposition  method  to  use.    There  are  currently
two options: 
EQ.“RCB”: 
recursive coordinate bisection 
EQ.“GREEDY”:  a simple heuristic method 
In  almost  all  cases  the  RCB  method  is  superior  and  should  be
used.
*CONTROL_MPP_DECOMPOSITION_NUMPROC 
Purpose:  Specify the number of processors for decomposition. 
2 
3 
4 
5 
6 
7 
8 
  Card 1 
Variable 
Type 
1 
N 
I 
Default 
none 
  VARIABLE   
DESCRIPTION
N 
Number of processors for decomposition. 
Remarks: 
This  is  used  in  conjunction  with  the  CONTROL_MPP_DECOMPOSITION_FILE 
command  to  allow  for  later  runs  on  different  numbers  of  processors.    By  default,  the 
decomposition  is  performed  for  the  number  of  processors  currently  being  used.  
However,  a  different  value  can  be  specified  here.    If  N > 1  and  only  one  processor  is 
currently being used, the decomposition is done and then the program terminates.  If N 
is  not  a  multiple  of  the  current  number  of  processors,  then  it  is  ignored  the  execution 
proceeds  with  the  current  number  of  processors.    Otherwise,  the  decomposition  is 
performed  for  N  processors,  and  the  execution  continues  using  the  current  number  of 
processors.
*CONTROL_MPP_DECOMPOSITION_OUTDECOMP 
Purpose:    Instructs  the  program  to  output  element's  ownership  data  to  file  for  post-
processor to show state data from different processors 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TYPE 
Type 
I 
Default 
none 
  VARIABLE   
DESCRIPTION
ITYPE 
Sets the format for the output file. 
EQ.1:  database in LS-PrePost format:  
decomp_parts.lsprepost. 
EQ.2:  database in animator format: 
decomp_parts.ses 
Remarks: 
Command in partition file (pfile): OUTDECOMP ITYPE. 
When ITYPE is set to 1, the elements assigned to any particular core can be viewed and 
animated  by    LS-PrePost  by  (1)  reading  the  d3plot  data,  and  then  (2)  selecting  
Models > Views > MPP > Load > decomp_parts.lsprepost.
*CONTROL_MPP_DECOMPOSITION_PARTS_DISTRIBUTE_OPTION 
Purpose:    Distribute  the  parts  given  in  this  option  to  all  processors  before  the 
decomposition for the rest of the model is performed.  If this appears in an included file 
and  the  LOCAL  option  is  given,  the  decomposition  will  be  done  in  the  coordinate 
system of the included file, which may be different from the global system if the file is 
included via *INCLUDE_TRANSFORM. 
  Card 1 
1 
Variable 
ID1 
2 
ID2 
3 
ID3 
4 
ID4 
5 
ID5 
6 
ID6 
7 
ID7 
8 
ID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
ID1, ID2, 
ID3, … 
DESCRIPTION
For each ID: 
GT.0: ID is a part number. 
LT.0:  –ID is a part set number. 
All parts defined in this card will be treated as a single region to
be decomposed. 
Remarks: 
Up  to  16  parts/part  sets  can  be  specified.    The  decomposition  is  modified  as  follows:  
the elements involved in the given parts are put into a separate domain from rest of the 
model and then distributed to all processors to balance their computational cost.  Then 
the remainder of the model will be distributed in the usual way. 
This is equivalent to the pfile command (for example, if ID1-ID3 are part ids and ID4-
ID6 are partset ids): 
            decomp { region { parts ID1 ID2 ID3 or partsets ID4 ID5 ID6 } } 
(the partset ids are positive when used in the pfile).
*CONTROL_MPP_DECOMPOSITION_PARTSET_DISTRIBUTE_OPTION 
Purpose:    Distribute  the  part  sets  given  in  this  option  to  all  processors  before  the 
decomposition  for  the  remainder  of  the  model  is  performed.  If  this  appears  in  an 
included  file  and  the  LOCAL  option  is  given,  the  decomposition  will  be  done  in  the 
coordinate system of the included file, which may be different from the global system if 
the file is included via *INCLUDE_TRANSFORM. 
  Card 1 
1 
Variable 
ID1 
2 
ID2 
3 
ID3 
4 
ID4 
5 
ID5 
6 
ID6 
7 
ID7 
8 
ID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
DESCRIPTION
Partset  ID  to  be  distributed..    All  parts  in  ID1  will  be  shared
across  all  processors.    Then  all  parts  in  ID2  will  be  distributed,
and so on.. 
  VARIABLE   
ID1, ID2, 
ID3, … 
Remarks: 
Any  number  of  part  sets  can  be  specified.    Each  part  set  is  distributed  across  all 
processors, in the order given.  The order may be significant, in particular, if a part ID is 
in  more  than  one  set.    Distribution  of  these  parts  is  done  before  any  decomposition 
specifications given in the pfile.
*CONTROL_MPP_DECOMPOSITION_RCBLOG 
Purpose:  Causes the program to record decomposition information in the indicated file, 
for use in subsequent analyses. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
FILENAME 
A80 
none 
DESCRIPTION
Name  of  output  file  where  decomposition  history  will  be
recorded.  This file can be used as the pfile for later analyses. 
Variable 
Type 
Default 
  VARIABLE   
FILENAME 
Remarks: 
Command in parallel option file (pfile): rcblog filename.
*CONTROL_MPP_DECOMPOSITION_SCALE_CONTACT_COST 
Purpose:  Instructs the program to apply a scale factor to the list of contacts to change 
the partition weight for the decomposition. 
  Card 1 
Variable 
1 
SF 
2 
ID1 
3 
ID2 
4 
ID3 
5 
ID4 
6 
ID5 
7 
ID6 
8 
ID7 
Type 
F 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
SF 
Scale factor for the contact segments listed in the interface ID. 
ID1, ID2, … 
interfaces ID's to be considered for scaling.  Include second card if
necessary. 
Remarks: 
Up  to  15  contact  interfaces  ID  can  be  specified.    The  decomposition  is  modified  by 
applying  this  scale  factor  to  the  default  computational  cost  of  elements  for  the  given 
contact interface ID. 
Command in partition file (pfile): CTCOST ID1, ID2, …, SF.
*CONTROL_MPP_DECOMPOSITION_SCALE_FACTOR_SPH 
Purpose:    Instructs  the  program to  apply  a  scale  factor  to SPH  elements  to  change the 
partition weight for the decomposition. 
2 
3 
4 
5 
6 
7 
8 
  Card 1 
Variable 
1 
SF 
Type 
F 
Default 
none 
  VARIABLE   
DESCRIPTION
SF 
Scale factor 
Remarks: 
Command in partition file (pfile): SPHSF SF.
*CONTROL_MPP_DECOMPOSITION_SHOW 
Purpose:  The keyword writes the final decomposition to the d3plot database.  There are 
no input parameters. 
This keyword causes MPP LS-DYNA to terminate immediately after the decomposition 
phase  without  performing  an  analysis.    The  resulting  d3plot  database  is  designed  to 
allow visualization of the decomposition by making each part correspond to the group 
of solids, shells, beams, thick shells, or SPH particles assigned to a particular processor.  
For  example,  in  a  model  that  includes  various  element  types  including  solids,  part  1 
corresponds  to  the  solid  elements  assigned  to  processor  1,  part  2  corresponds  to  the 
solid elements assigned to processor 2, and so on. 
This  command  can  be  used  in  conjunction  with  the  *CONTROL_MPP_DECOMPOSI-
TION_NUMPROC  command  to  run  on  one  processor  and  produce  a  d3plot  file  to 
visualize the resulting decomposition for the number of processors specified in *CON-
TROL_MPP_DECOMPOSITION_NUMPROC.
*CONTROL_MPP_DECOMPOSITION_TRANSFORMATION 
Purpose:  Specifies transformations to apply to modify the decomposition. 
There are 10 different kinds of decomposition transformations available.  For a detailed 
description of each, see Appendix O the LS-DYNA MPP user guide. 
The data cards for this keyword consist of transformation operations.  Each operation, 
depending on its type, involves either one or two additional cards.  The input deck may 
include  an  arbitrary  number  of  transformations  with  the  next  keyword,  “*,”  card 
terminating this input. 
Transformation Card 1.  For each transformation this card is required. 
  Card 1 
1 
Variable 
TYPE 
2 
V1 
Type 
A10 
F 
3 
V2 
F 
4 
V3 
F 
5 
V4 
F 
6 
V5 
F 
7 
V6 
F 
8 
Default 
none 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Transformation Card 2.  Additional card for TYPE set to one of VEC3, C2R, S2R, MAT.
4 
5 
6 
7 
8 
  Card 2 
Variable 
1 
V7 
Type 
F 
2 
V8 
F 
3 
V9 
F 
Default 
0.0 
0.0 
0.0 
  VARIABLE   
TYPE 
DESCRIPTION
Which transformation to apply.  The allowed values are RX, RY,
RZ, SX, SY, SZ, VEC3, C2R, S2R, and MAT.
VARIABLE   
DESCRIPTION
V1 - V9 
For type set to either RX, RY, RZ, SX, SY, or SZ: 
The  parameter  V1  gives  either  the  angle  of  rotation  (RX,
RY, RZ) or the magnitude for the scaling (SX, SY, SZ).  The
remaining parameters are ignored. 
For type set to either VEC3, C2R, S2R, or MAT: 
All parameters are used.  See the appendix for the “pfile.”
*CONTROL_MPP_IO_LSTC_REDUCE 
Purpose:  Use LSTC's own reduce routine to get consistent summation of floating point 
data among processors.  There are no input parameters. 
Remarks: 
Command in partition file (pfile): lstc_reduce.
*CONTROL_MPP_IO_NOBEAMOUT 
Purpose:    Suppress  beam,  shell,  and  solid  element  failure  messages  in  the  d3hsp  and 
message files.  There are no parameters for this keyword. 
Remarks: 
Command in parallel option file (pfile): nobeamout.
*CONTROL_MPP_IO_NOD3DUMP 
Purpose:  Suppresses the output of all dump files. 
There are no input parameters.  The existence of this keyword causes the d3dump and 
runrsf file output routines to be skipped.
*CONTROL_MPP_IO_NODUMP 
Purpose:  Suppresses the output of all dump files and full deck restart files. 
There are no input parameters.  The existence of this keyword causes the d3dump and 
runrsf  file  output  routines  to  be  skipped.    It  also  suppresses  output  of  the  full  deck 
restart file d3full.
*CONTROL 
Purpose:    Turn  off  failed  element  checking  in  MPP  contact.    If  you  know  that  no 
elements  will  fail,  or  that  any  such  failure  will  not  impact  any  of  the  contact 
calculations, turning on this option can increase the efficiency of the contact routines. 
There are no input parameters.
*CONTROL_MPP_IO_NOFULL 
Purpose:  Suppresses the output of the full deck restart files. 
There are no input parameters.  The existence of this keyword suppresses the output of 
the full deck restart file d3full.
*CONTROL_MPP_IO_SWAPBYTES 
Purpose:  Swap bytes on some of the output files. 
There are no input parameters.  The existence of this keyword causes the d3plot file and 
the  “interface  component  analysis”  file  to  be  output  with  bytes  swapped.    This  is  to 
allow  further  processing  of  data  on  a  different  machine  that  has  big  endian  vs.    little 
endian incompatibilities compared to the system on which the analysis is running.
*CONTROL_MPP_MATERIAL_MODEL_DRIVER 
Purpose:    Enable  this  feature  in  MPP  mode.    To  allow  MPP  reader  to  pass  the  input 
phase even without any nodes and elements but using only one processor.
*CONTROL_MPP_PFILE 
Purpose:  Provide keyword support for the MPP “p=” pfile options 
All lines of input up to the next keyword card will be copied to a temporary file which 
is  effectively  pre-pended  to  the  “p=”  file  given  on  the  command  line  (even  if  no  such 
file  is  given).    This  allows  all  options  available  via  the  “p=”  file  to  be  specified  in  the 
keyword input.  The only restriction is that pfile directives in the “directory” section are 
not available, as those must be processed before the keyword input file is read.  See the 
“LS-DYNA  MPP  User  Guide”  in  the  appendix  for  details  of  the  available  pfile 
commands and their syntax.
*CONTROL_NONLOCAL 
Purpose:  Allocate additional memory for *MAT_NONLOCAL option. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MEM 
Type 
I 
Default 
none 
  VARIABLE   
MEM 
DESCRIPTION
Percentage increase of memory allocated for *MAT_NONLOCAL 
option  over  that required  initially.    This  is  for  additional  storage
that may be required due to geometry changes as the calculation
proceeds.  Generally, a value of 10 should be sufficient.
*CONTROL 
Purpose:    Set  miscellaneous  output  parameters.    This  keyword  does  not  control  the 
information,  such  as  the  stress  and  strain  tensors,  which  is  written  into  the  binary 
databases.  For the latter, see the keyword *DATABASE_EXTENT_BINARY. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NPOPT 
NEECHO  NREFUP 
IACCOP 
OPIFS 
IPNINT 
IKEDIT 
IFLUSH 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
F 
0. 
I 
0 
I 
I 
100 
5000 
Remaining cards are optional. 
Optional Card 2 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IPRTF 
IERODE 
TET10S8 MSGMAX
IPCURV 
GMDT 
IP1DBLT 
EOCS 
Type 
Default 
I 
0 
I 
0 
I 
2 
I 
50 
I 
0 
F 
0. 
I 
0 
I 
0 
Optional Card 3 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TOLEV 
NEWLEG 
FRFREQ  MINFO 
SOLSIG  MSGFLG  CDETOL 
Type 
Default 
I 
2 
I 
0 
I 
1 
I 
0 
I 
0 
I 
0 
F 
10.0
*CONTROL_OUTPUT 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  PHSCHNG  DEMDEN 
Type 
Default 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
NPOPT 
Print suppression during input phase flag for the “d3hsp” file: 
EQ.0: no suppression, 
EQ.1: nodal  coordinates,  element  connectivities,  rigid  wall
definitions,  nodal  SPCs,  initial  velocities,  initial  strains,
adaptive constraints, and SPR2/SPR3 constraints are not
printed. 
NEECHO 
Print suppression during input phase flag for “echo” file: 
EQ.0: all data printed, 
EQ.1: nodal printing is suppressed, 
EQ.2: element printing is suppressed, 
EQ.3: both node and element printing is suppressed. 
NREFUP 
Flag to update reference node coordinates for beam formulations
1,  2,  and  11.    This  option  requires  that  each  reference  node  is
unique to the beam: 
EQ.0: Do not update reference node.  
EQ.1: Update reference node:  This  update 
is  required  for 
proper  visualization  of  the  beam  cross-section  orienta-
tion  in  LS-PrePost  beyond  the  initial  (𝑡 = 0)  plot  state. 
NREFUP  does  not  affect  the  internal  updating  of  the
beam cross-section orientation in LS-DYNA.
VARIABLE   
IACCOP 
OPIFS 
IPNINT 
IKEDIT 
IFLUSH 
DESCRIPTION
Flag  to  average  or  filter  nodal  accelerations  output  to  file
“nodout” and the time history database “d3thdt”: 
EQ.0: no average (default), 
EQ.1: averaged between output intervals, 
EQ.2: accelerations for each time step are stored internally and
then filtered over each output interval using a filter from
General Motors [Sala, Neal, and Wang, 2004] based on a
low-pass  Butterworth  frequency  filter.    See  also  [Neal,
Lin,  and  Wang,  2004]. 
in  *CONTROL_-
TIMESTEP  must  be  set  to  a  negative  value  when  IAC-
COP = 2  so  that  the  maximum  possible  number  of  time
steps  for  an  output  interval  is  known  and  adequate 
memory can be allocated.  See Figure 12.15. 
  DT2MS 
Output time interval for interface file written per *INTERFACE_-
COMPONENT_option. 
Flag  controlling  output  of  initial  time  step  sizes  for  elements  to
“d3hsp”: 
EQ.0: 100  elements  with  the  smallest  time  step  sizes  are
printed. 
EQ.1: Time step sizes for all elements are printed. 
GT.1:  IPNINT  elements  with  the  smallest  time  step  sizes  are
printed. 
Problem status report interval steps to the “d3hsp” file.  This flag 
is  ignored  if  the  “glstat”  file  is  written,  see  *DATABASE_GL-
STAT. 
Number  of  time  steps  interval  for  flushing  I/O  buffers.    The 
default  value  is  5000.    If  the  I/O  buffers  are  not  emptied  and  an
abnormal termination occurs, the output files can be  incomplete.
The  I/O  buffers  for  restart  files  are  emptied  automatically
whenever a restart file is written so these files are not affected by 
this option.
IPRTF 
*CONTROL_OUTPUT 
DESCRIPTION
Default  print  flag  for  “rbdout”  and  “matsum”  files.    This  flag 
defines  the  default  value  for  the  print  flag  which  can  be  defined
in the part definition section, see *PART.  This option is meant to
reduce the file sizes by eliminating data which is not of interest. 
EQ.0: write part data into both matsum and rbdout 
EQ.1: write data into rbdout file only 
EQ.2: write data into matsum file only 
EQ.3: do not write data into rbdout and matsum 
IERODE 
Output eroded internal and kinetic energy into the “matsum” file. 
Also, output to the “matsum” file under the heading of part ID 0 
is  the  kinetic  energy  from  nonstructural  mass,  lumped  mass
elements and lumped inertia elements.   
TET10S8 
EQ.0: do not output extra data 
EQ.1: output the eroded internal and kinetic energy 
Output  ten  connectivity  nodes  for  the  10-node  solid  tetrahedral 
and  the  eight  connectivity  nodes  for  the  8-node  shell  into 
“d3plot”  database.    The  current  default  is  set  to  2  since  this
change  in  the  database  may  make  the  data unreadable  for  many
popular  post-processors  and  older  versions  of  LS-PrePost.    The 
default will change to 1 later. 
EQ.1: write  the  full  node  connectivity  into  the  “d3plot” 
database 
EQ.2: write  only  the  corner  nodes  of  the  elements  into  the 
“d3plot” database 
MSGMAX 
Maximum number of each error/warning message 
GT.0:  number  of  messages  to  screen  output,  all  messages
written to d3hsp/messag 
LE.0:  number 
of  messages 
to 
screen 
output 
and 
d3hsp/messag 
EQ.0: default, 50 
IPCURV 
Flag to output digitized curve data to “messag” and d3hsp files. 
EQ.0: off 
EQ.1: on
VARIABLE   
GMDT 
DESCRIPTION
Output  interval  for  recorded  motions  from  *INTERFACE_SSI_-
AUX 
IP1DBLT 
Output information of 1D (bar-type) seatbelt created for 2D (shell-
type) seatbelt to sbtout.   
EQ.0: the analysis results of internally created 1D seatbelts are
extracted and processed to yield the 2D belt information.
The 2D belt information is stored in sbtout, 
EQ.1: the  analysis  results  of  internally  created  1D  retractors
and  slip  rings  are  stored  in  sbtout.    Belt  load  can  be 
yielded by *DATABASE_CROSS_SECTION. 
EOCS 
Elout  Coordinate  System:  controls  the  coordinate  system  to  be
used when writing out shell data to the “elout” file: 
EQ.0: default 
EQ.1: local element coordinate system 
EQ.2: global coordinate system 
TOLEV 
NEWLEG 
FRFREQ 
Timing  Output  Levels:  controls  the  #  of  levels  output  in  the
timing summary at termination.  The default is 2. 
New  Legends:  controls  the  format  of  the  LEGEND  section  of
various ASCII output files. 
EQ.0: use the normal format 
EQ.1: use the optional format with extra fields. 
Output frequency for failed element report, in cycles.  The default
is  to  report  the  summary  every  cycle  on  which  an  element  fails. 
If > 1,  the  summary  will  be  reported  every  FRFREQ  cycles
whether an element fails that cycle or not, provided some element
has  failed  since  the  last  summary  report.    Individual  element
failure is still reported as it occurs. 
MINFO 
Output  penetration  information  for  mortar  contact  after  each
implicit  step,  not  applicable  in  explicit  analysis.    See  remarks  on
mortar contact on *CONTACT card. 
EQ.0: No information 
EQ.1: Penetrations reported for each contact interface.
SOLSIG 
MSGFLG 
CDETOL 
*CONTROL_OUTPUT 
DESCRIPTION
Flag to extrapolate stresses and other history variables for multi-
integration point solids from integration points to nodes.   These
extrapolated  nodal  values  replace  the  integration  point  values
normally  stored  in  d3plot.    When  a  nonzero  SOLSIG  is  invoked, 
NINTSLD  in  *DATABASE_EXTENT_BINARY  should  be  set  to  8 
as  any  other  value  of  NINTSLD  will  result  in  only  one  value
being  reported  for  each  element.    Supported  solid  formulations
are: -1, -2, 2, 3, 4, 18, 16, 17, and 23. 
NOTE: Do  not  use  "Setting  -  Extrapolate"  in  LS-
PrePost when this field, SOLSIG, is nonzero. 
EQ.0: No extrapolation. 
EQ.1: Extrapolate the stress for linear materials only. 
EQ.2: Extrapolate the stress if plastic strain is zero. 
EQ.3: Extrapolate the stress always. 
EQ.4: Extrapolate all history variables. 
Flag  for  writing  detailed  error/warning  messages  to  d3msg.
MSGFLG  has  no  affect  on 
length
error/warning messages; such messages are written to messag or
mes****.  NOTE: Most errors/warnings offer only standard length 
messages.  Only a few also offer optional, detailed messages.   
  output  of  standard 
EQ.0: Do not write detailed messages to d3msg. 
EQ.1: Write  detailed  messages  to  d3msg  at  the  conclusion  of
the run.  Each detailed message is written only once even
in  cases  where  the  associated  error  or  warning  occurs 
multiple times. 
for  output  of 
*DEFINE_CURVE  discretization 
Tolerance 
warnings.    After  each  curve  is  discretized,  the  resulting  curve  is
evaluated at each of the original definition points, and the values
compared.    A  warning  will  be  issued  for  any  curve  where  this
comparison  results  in  an  error  of  more  than  CDETOL/100 × 𝑀, 
where  the  curve  specific  value  𝑀  is  computed  as  the  median  of 
the absolute values of the non-zero curve values.
VARIABLE   
PHSCHNG 
DESCRIPTION
Message  to  messag  file  when  materials  216,  217,  and  218  change
phase.. 
EQ.0: (default) no message. 
EQ.1: The time and element ID are written. 
DEMDEN 
Output DEM density data to d3plot database.. 
EQ.0: (default) no output. 
EQ.1: output data.
*CONTROL_PARALLEL 
Purpose:  Control parallel processing usage  by defining the number of processors and 
invoking the optional consistency of the global vector assembly.  This command applies 
only  to  shared  memory  parallel  (SMP)  LS-DYNA.    It  does  not  apply  to  distributed 
memory parallel (MPP) LS-DYNA. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NCPU 
NUMRHS 
CONST 
PARA 
Type 
Default 
I 
1 
Remarks 
  VARIABLE   
NCPU 
I 
0 
1 
I 
2 
2 
I 
0 
3 
DESCRIPTION
Number of cpus used. 
(This  parameter  is  disabled  in  971  R5  and  later  versions.    Set
number  of  cpus  using  “ncpu=”  on  the  execution  line  —  see 
Execution  Syntax  section  of  Getting  Started  —  or    on  the 
*KEYWORD line of the input.) 
NUMRHS 
Number of right-hand sides allocated in memory: 
EQ.0: same as NCPU, always recommended, 
EQ.1: allocate only one. 
CONST 
Consistency  flag.    (Including  “ncpu=n”  on  the  execution  line  or 
on the *KEYWORD line of input overrides CONST.  The algebraic
sign of n determines the consistency setting.) 
EQ.1 or n < 0: 
EQ.2 or n > 0: 
on (recommended) 
off, for a faster solution (default).
VARIABLE   
PARA 
DESCRIPTION
Flag for parallel force assembly if CONST=1.  (Including “para=” 
on the execution line overrides PARA.) 
EQ.0: off 
EQ.1: on 
EQ.2: on 
Remarks: 
1. 
It is recommended to always set NUMRHS = NCPU since great improvements 
in the parallel performance are obtained since the force assembly is then done 
in  parallel.    Setting  NUMRHS  to  one  reduces  storage  by  one  right  hand  side 
vector  for  each  additional  processor  after  the  first.    If  the  consistency  flag  is 
active, i.e., CONST = 1, NUMRHS defaults to unity. 
2.  For  any given  problem  with  the  consistency  option  off,  i.e.,  CONST = 2,  slight 
differences in results are seen when running the same  job multiple times with 
the  same  number  of  processors  and  also  when  varying  the  number  of  proces-
sors.  Comparisons of nodal accelerations often show wide discrepancies; how-
ever,  it  is  worth  noting  that  the  results  of  accelerometers  often  show 
insignificant variations due to the smoothing effect of the accelerometers which 
are generally attached to nodal rigid bodies. 
The  accuracy  issues  are  not  new  and  are  inherent  in  numerical  simulations  of 
automotive  crash  and  impact  problems  where  structural  bifurcations  under 
compressive  loads  are  common.    This  problem  can  be  easily  demonstrated  by 
using  a  perfectly  square  thin-walled  tubular  beam  of  uniform  cross  section 
under a compressive load.  Typically, every run on one processor that includes 
a  minor  input  change  (i.e.,  element  or  hourglass  formulation)  will  produces 
dramatically  different  results  in  terms  of  the  final  shape,  and,  likewise,  if  the 
same problem is again run on a different brand of computer.  If the same prob-
lem is run on multiple processors the results can vary dramatically from run to 
run WITH NO INPUT CHANGE.  The problem here is due to the randomness 
of numerical round-off which acts as a trigger in a “perfect” beam. 
Since summations with (CONST=2) occur in a different order from run to run, 
the  round-off  is  also  random.    The  consistency  flag,  CONST=1,  provides  for 
identical  results  (or  nearly  so)  whether  one,  two,  or  more  processors  are  used 
while  running  in  the  shared  memory  parallel  (SMP)  mode.    This  is  done  by 
requiring that all contributions to global vectors be summed in a precise order 
independently of the number of processors used.  When checking for consistent 
results,  nodal  displacements  or  element  stresses  should  be  compared.    The
NODOUT  and  ELOUT  files  should  be  digit  to  digit  identical.    However,  the 
GLSTAT,  SECFORC,  and  many  of  the  other  ASCII  files  will  not  be  identical 
since the quantities in  these files are summed in parallel for efficiency reasons 
and the ordering of summation operations are not enforced.  The biggest draw-
back  of  this  option  is  the  CPU  cost  penalty  which  is  at  least  15  percent  if  PA-
RA=0 and is much less if PARA=1 and 2 or more processors are used.  Unless 
the  PARA  flag  is  on  (for  non-vector  processors),  parallel  scaling  is  adversely 
affected.  The consistency flag does not apply to MPP parallel. 
3.  PARA set to 1 or 2 will cause the force assembly for the consistency option to be 
performed  in  parallel  for  the  SMP  version,  so  better  scaling  will  be  obtained.  
However,  PARA = 1  will  increase  memory  usage  while  PARA = 2  will  not.  
This  flag  does  not  apply  to  the  MPP  version.    If  PARA = CONST = 0  and 
NUMRHS = NCPU the force assembly by default is done in parallel, but with-
out  consistency.    The  value  of  the  flag  may  also  be  given  by  including  “pa-
ra=<value>”  on  the  execution  line,  and  the  value  given  in  this  manner  will 
override the value of PARA in *CONTROL_PARALLEL.
*CONTROL 
Purpose:  Set parameters for pore water pressure calculations. 
This  control  card  is  intended  for  soil  analysis.    However,  other  materials  containing 
pore  fluid  could  be  treated  by  the  same  methods.    The  pore  pressure  capabilities 
invoked by this card are available in SMP and MPP versions of LS-DYNA, but are not 
available for implicit solutions.  Furthermore, pore pressure capabilities are limited to a 
subset of 3-D solid Lagrangian element formulations, including solid formulations 1, 2, 
4, 10, and 15. 
LS-DYNA uses Terzaghi’s Effective Stress to model materials with pore pressure.  The 
pore fluid and soil skeleton are assumed to occupy the same volume and to carry loads 
in parallel.  Thus, the total stress in an element is the sum of the “effective stress” in the 
soil  skeleton,  plus  the  hydrostatic  stress  in  the  pore  fluid.    LS-DYNA  calculates  the 
“effective  stress”  with  standard  material  models.      The  pore  fluid  treatment,  then,  is 
independent  of  material  model.    The  pore  pressure  is  calculated  at  nodes,  and 
interpolated  onto  the  elements.    The  pore  fluid’s  hydrostatic  stress  is  equal  to  the 
negative of the element pore pressure. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ATYPE 
(blank)  WTABLE 
PF_RHO 
GRAV 
PF_BULK  OUTPUT 
TMF 
Type 
Default 
I 
0 
F 
F 
F 
F 
F 
0.0 
0.0 
(none) 
(none) 
(none) 
  Card 2 
1 
2 
3 
4 
5 
6 
I 
0 
7 
F 
1.0 
8 
Variable 
TARG 
FMIN 
FMAX 
FTIED 
CONV 
CONMAX 
ETERM 
THERM 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
1.E-4 
1.E20 
0.0 
0.0
*CONTROL_PORE_FLUID 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ETFLAG 
Type 
Default 
I 
0 
  VARIABLE   
DESCRIPTION
ATYPE 
Analysis type for pore water pressure calculations: 
EQ.0: No pore water pressure calculation. 
EQ.1: Undrained analysis, 
EQ.2: Drained analysis,  
EQ.3: Time dependent consolidation (coupled), 
EQ.4: Consolidate to steady state (uncoupled), 
EQ.5: Drained in dynamic relaxation, undrained in transient, 
EQ.6: As 4 but do not check convergence, continue to end time.
WTABLE 
Default z-coordinate of water table (where pore pressure is zero).  
PF_RHO 
Default density for pore water. 
GRAV 
Gravitational  acceleration  used  to  calculate  hydrostatic  pore 
water pressure. 
PF_BULK 
Default bulk modulus of pore fluid (stress units).   
OUTPUT 
Output  flag  controlling  stresses  to  D3PLOT  and  D3THDT  binary 
files: 
EQ.0: total stresses are output 
EQ.1: effective stresses are output, see notes
VARIABLE   
DESCRIPTION
TMF 
Initial Time Magnification factor on seepage (ATYPE = 3,4 only).  
TARG 
FMIN 
FMAX 
FTIED 
CONV 
GT.0: Factor  (can  be  used  with  automatic  control,  see  TARG,
FMIN, FMAX). 
LT.0:  Load  Curve  ID    giving  Time 
Magnification Factor versus analysis time.   
Target for maximum change of excess pore pressure at any node,
per timestep.  If the actual change falls below the target, the time
factor on the seepage calculation will be increased .  If
zero, the constant value of TMF is used.  If non-zero, TMF is taken 
as the initial factor. 
Minimum time factor on seepage calculation 
Maximum time factor on seepage calculation 
Analysis type for pore water pressure calculations: 
EQ.0.0: Tied contacts act as impermeable membranes, 
EQ.1.0: Fluid may flow freely through tied contacts. 
Convergence  tolerance  for  ATYPE = 4.    Maximum  head  change 
per  time  step  at  any  node  as  measured  in  units  of  characteristic
length, l. 
𝑙 =
𝜌𝑔
where, 
𝜌 = pore fluid density, PF_ RHO 
𝑔 = gravitational acceleration. 
CONMAX 
Maximum factor on permeability with ATYPE = -4 
ETERM 
Event time termination (ATYPE = 3) 
THERM 
Thermal  expansion:    Volumetric  strain  per  degree  increase  for
undrained soil. 
ETFLAG 
Flag for interpretation of time etc : 
EQ.0: Time means analysis time, 
EQ.1: Time means event time.
Undrained 
*CONTROL_PORE_FLUID 
For analyses of the “undrained” type the pore fluid is trapped within the materi-
al.  Volume changes result in pore pressure changes.  This approximation is used 
to simulate the effect of rapidly-applied loads on relatively impermeable soil. 
Drained 
For  analyses  of  the  “drained”  type  the  pore  fluid  is  free  to  move  within  the 
material  such  that  the  user-defined  pressure-versus-z-coordinate  relationship  is 
always  maintained.    This  approximation  is  used  to  model  high-permeability 
soils. 
Time-dependent consolidation 
For  the  analysis  type  “time  dependent  consolidation,”  pressure  gradients  cause 
pore fluid to flow through the material according to Darcy’s law:  
where, 
v = κ∇(p + z) 
v = fluid velocity vector 
κ = permeability 
p = pressure head 
z = z-coordinate. 
Net inflow or outflow at a node leads to a theoretical volume gain or loss.  The 
analysis  is  coupled,  i.e.    any  difference  between  actual  and  theoretical  volume 
leads to pore pressure change, which in turn affects the fluid flow.  The result is a 
prediction of response-versus-time. 
Steady-state consolidation 
For the analysis type “steady-state consolidation,” an iterative method is used to 
calculate the steady-state pore pressure.  The analysis is uncoupled, i.e.  only the 
final state is meaningful, not the response-versus-time.    
Time factoring: 
Consolidation  occurs  over  time  intervals  of  days,  weeks  or  months.    To  simulate  this 
process  using  explicit  time  integration,  a  time  factor  is  used.    The  permeability  of  the 
soil  is  increased  by  the  time  factor  so  that  consolidation  occurs  more  quickly.    The 
output  times  in  the  D3PLOT  and  D3THDT  files  are  modified  to  reflect  the  time  factor.  
The factored  time (“Event Time”) is intended to represent the time taken in the real-life 
consolidation  process  and  will  usually  be  much  larger  than  the  analysis  time  (the 
analysis  time  is  the  sum  of  the  LS-DYNA  timesteps).    The  time  factor  may  be  chosen
explicitly  (using  TMF)  but  it  is  recommended  to  use  automatic  factoring  instead.    The 
automatic scheme adjusts the time factor according to how quickly the pore pressure is 
changing;  usually  at  the  start  of  consolidation  the  pore  pressure  changes  quickly  and 
the  time  factor  is  low;  the  time  factor  increases  gradually  as  the  rate  of  pore  pressure 
change  reduces.    Automatic  time  factoring  is  input  by  setting  TARG  (the  target  pore 
pressure  head  change  per  timestep)  and  maximum  and  minimum  allowable  time 
factors,  for  example  TARG  =  0.001  to  0.01m  head,  FMIN  =  1.0,  FMAX  =  1.0e6.  
Optimum settings for these are model-dependent.  
Loading, other input data from loadcurves, and output time-intervals on *DATABASE 
cards by default use the analysis time (for example, the x-axis of  a loadcurve used  for 
pressure  loading  is  analysis  time).    When  performing  consolidation  with  automatic 
time-factoring, the relationship between analysis time and event time is unpredictable.  
Termination based on event time may be input using ETERM.  
It  may  also  be  desired  to  apply  loads  as  functions  of  event  time  rather  than  analysis 
time,  since  the  event  time  is  representative  of  the  real-life  process.    By  setting 
ETFLAG = 2, the time axis of all load curves used for any type of input-versus-time, and 
output intervals on *DATABASE cards, will be interpreted as event time.  This method 
also allows  consolidation to be used as part of a staged construction sequence – when 
ETFLAG = 2, the stages begin and end at the “real time” stage limits and input curves of 
pore pressure analysis type vs.  time may be used to enforce, for example, consolidation 
in some stages, and undrained behavior in others. 
Output: 
Extra  variables  for  solid  elements  are  automatically  written  to  the  d3plot  and  d3thdt 
files  when  the  model  contains  *CONTROL_PORE_FLUID.    In  LS971  R4  onwards,  5 
additional  extra  variables  are  written,  of  which  the  first  is  the  pore  pressure  in  stress 
units.    In  LS971  R3,  15  additional  extra  variables  are  written,  of  which  the  seventh  is 
pore  pressure  in  stress  units.    These  follow  any  extra  variables  requested  by  the  user, 
e.g.  if the user requested 3 extra variables, then in LS971 there will be a total of 8 extra 
variables of which the fourth is pore pressure.  
Further  optional  output  to  d3plot  and  d3thdt  files  is  available  for  nodal  pore  pressure 
variables – see *DATABASE_PWP_OUTPUT. 
For time-dependent and steady-state consolidation, information on the progress of the 
analysis is written to d3hsp file.  
Remarks: 
1.  Tied Contacts.  By default, the mesh discontinuity at a tied contact will act as a 
barrier to fluid flow.  If the flag FTIED is set to 1, then pore fluid will be trans-
mitted  across  tied  nodes  in  tied  contacts  (*CONTACT_TIED_SURFACE_TO_-
SURFACE  and  *CONTACT_TIED_NODES_TO_SURFACE,  including_OFFSET 
and non-_OFFSET types).  This algorithm has an effect only when the analysis 
type of at least one of the contacting parts is 3, 4 or 6. 
2.  Thermal.  Note that this property is for VOLUMETRIC strain increase.  Typical 
thermal expansion coefficients are linear; the volumetric expansion will be three 
times  the  linear  thermal  expansion  coefficient.    Regular  thermal  expansion 
coefficients (e.g.  on *MAT or *MAT_ADD_THERMAL_EXPANSION) apply to 
the  soil  skeleton  and  to  drained  parts.    Pore  pressure  can  be  generated  due  to 
the difference of expansion coefficients of the soil skeleton and pore fluid. 
3.  Part  Associativity.    Pore  pressure  is  a  nodal  variable,  but  analysis  type  and 
other  pore  pressure  related  inputs  are  properties  of  parts.    When  a  node  is 
shared by elements of different parts, and those parts have different pore pres-
sure inputs, the following rules are followed to determine which part’s proper-
ties should be applied to the node. 
a)  Dry  parts  (i.e.    parts  without  a  *BOUNDARY_PORE_FLUID  card)  will 
never be used (lowest priority). 
b)  If  a  part  is  initially  dormant  (due  to  staged  construction  inputs),    it  has 
next-lowest priority 
c)  Parts with analysis type = drained have highest priority.  
d)  Next, higher permeability gives higher priority 
e)  If  two  or  more  parts  have  equal-highest  priority  at  a  node, the  part  with 
lowest ID will win. 
4.  Related Cards: 
*BOUNDARY_PORE_FLUID. 
(This card is essential since without this card, no parts will have pore flu-
id.) 
*BOUNDARY_PWP_OPTION 
*DATABASE_PWP_OUTPUT 
*DATABASE_PWP_FLOW 
*MAT_ADD_PERMEABILITY
*CONTROL 
Purpose:  Set parameters for pore air pressure calculations. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
AIR_RO 
AIR_P 
ETERM 
ANAMSG 
Type 
F 
F 
F 
Default 
(none) 
(none) 
endtim 
I 
0 
  VARIABLE   
DESCRIPTION
PA_RHO 
Density of atmospheric air, = 1.184 kg/m3 at 25°C 
PA_PATM 
Pressure of atmospheric air, = 101.325 kPa at 25°C 
ETERM 
ANAMSG 
Event  termination  time,  default  to  ENDTIME  of  *CONTROL_-
TERMINATION 
Flag  to  turn  off  the  printing  of  pore  air  analysis  status  message,
including  the  analysis  time,  the  node  with  the  highest  pressure
change. 
EQ.0:  Status messages are printed, the default value. 
EQ.1:  Status messages are not printed
*CONTROL_REFINE_ALE 
Purpose:    Refine  ALE  hexahedral  solid  elements  locally.    Each  parent  element  is 
replaced  by  8  child  elements  with  a  volume  equal  to  1/8th  the  parent  volume.   If  only 
the  1st  card  is  defined,  the  refinement  occurs  during  the  initialization.    The  2nd  card 
defines a criterion CRITRF to automatically refine the elements during the run.  If the 3rd 
card  is  defined,  the  refinement  can  be  removed  if  a  criterion  CRITRM  is  reached:  the 
child elements can be replaced by their parents. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
TYPE 
NLVL 
MMSID 
IBOX 
IELOUT 
Type 
I 
Default 
none 
I 
0 
I 
1 
I 
0 
I 
0 
I 
0 
Remaining cards are optional.† 
Automatic  refinement  card.    Optional  card  for  activating  automatic  refinement 
whereby  each  element  satisfying  certain  criteria  is  replaced  by  a  cluster  of  8  child 
elements 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NTOTRF  NCYCRF 
CRITRF 
VALRF 
BEGRF 
ENDRF 
LAYRF 
DELAYRF
Type 
Default 
I 
0 
F 
0.0 
I 
0 
F 
F 
F 
0.0 
0.0 
0.0 
I 
0 
F 
0.0
Automatic  Refinement  Remove  Card.    Optional  card  for  activating  automatic 
refinement removal whereby, when, for a cluster of 8 child elements, certain criteria are 
satisfied the clusters is replaced by its parent. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MAXRM  NCYCRM  CRITRM 
VALRM 
BEGRM 
ENDRM  MMSRM  DELAYRM
Type 
Default 
I 
0 
F 
0.0 
I 
0 
F 
F 
F 
0.0 
0.0 
0.0 
I 
0 
F 
0.0 
  VARIABLE   
DESCRIPTION
ID 
Set ID. 
TYPE 
Set type: 
EQ.0: ALE Part Set, 
EQ.1: ALE Part, 
EQ.2: Lagrangian  Part  Set  coupled  to  ALE  , 
EQ.3: Lagrangian Part coupled to ALE , 
EQ.4: Lagrangian  Shell  Set  coupled  to  ALE  , 
EQ.5: ALE Solid Set. 
NLVL 
Number of refinement levels .  
MMSID 
Multi-Material Set ID  : 
LT.0:  only  ALE  elements  with  all  the  multi-material  groups 
listed in *SET_MULTI-MATERIAL_GROUP_LIST can be 
refined (or removed otherwise) 
GT.0: ALE  elements  with  at  least  one  of  the  multi-material 
groups can be refined (or removed) 
IBOX 
Box  ID    defining  a  region  in  which  the  ALE 
elements are refined. 
IELOUT 
Flag to handle child data in elout .
VARIABLE   
DESCRIPTION
NTOTRF 
Total number of ALE elements to refine : 
GT.0: Number of elements to refine 
EQ.0: NTOTRF = number  of  solid  elements  in  IBOX   
LT.0:  |NTOTRF| is the id of *CONTROL_REFINE_MPP_DIS-
TRIBUTION that computes the number of extra elements
required by processors. 
NCYCRF 
Number of cycles between each refinement. 
LT.0:  |NCYCRF| is the time interval 
CRITRF 
Refinement criterion:  
EQ.0: static refinement (as if only the 1st card is defined), 
EQ.1: Pressure (if pressure > VALRF), 
EQ.2: Relative Volume (if V/Vo < VALRF)  , 
EQ.3: Volume Fraction (if Volume fraction > VALRF),  
EQ.5: User  defined  criterion.    The  fortran  routine  alerfn_
criteria5  in  the  file  dynrfn_user.f  should  be  used  to  de-
velop the criterion.  The file is part of the general package
usermat.  
VALRF 
Criterion value to reach for the refinement. 
BEGRF 
Time to begin the refinement. 
ENDRF 
Time to end the refinement. 
LAYRF 
Number of element layers to refine around a element reaching the
refinement criterion . 
DELAYRF 
Period  of  time  after  removing  the  refinement  of  an  element,
during which this element will not be refined again. 
MAXRM 
Maximum number of child clusters to remove : 
LT.0:  for the whole run, 
GT.0: every NCYCRM cycles
VARIABLE   
DESCRIPTION
NCYCRM 
Number of cycles between each check for refinement removal: 
LT.0:  |NCYCRM| is the time interval 
CRITRM 
Criterion for refinement removal:  
EQ.0: no  refinement  removal  (as  if  only  the  1st  and  2nd  card
are defined), 
EQ.1: Pressure (if pressure < VALRM), 
EQ.2: Relative Volume (if V/Vo > VALRM)  , 
EQ.3: Volume Fraction (if Volume fraction < VALRM),  
EQ.5: User  defined  criterion.    The  fortran  routine  alermv_
criteria5 in the file dynrfn_user.f should be used to devel-
op  the  criterion.    The  file  is  part  of  the  general  package
usermat. 
VALRM 
Criterion  value  to  reach  in  each  child  element  of  a  cluster  for  its
removal (child elements replaced by parent element).. 
BEGRM 
Time to begin the check for refinement removal: 
LT.0:  |BEGRM| represents a critical percent of NTOTRF below
which  the  check  for  refinement  removal  should  begin
(0.0 < |BEGRM| < 1.0).  . 
ENDRM 
Time to end the check for refinement removal. 
MMSRM 
Multi-Material Set ID for the refinement removal.  
LT.0:  |  MMSRM  |  represents  the  radius  of  a  sphere  centered
on a newly refined element, in which the refinement can
not be removed. 
DELAYRM 
Period  of  time  after  refining  an  element,  during  which  this
refinement will not be removed. 
Remarks: 
1. 
2. 
If only the 1st card is defined, only TYPE = 0, 1, 5 can be defined.  
*CONSTRAINED_LAGRANGE_IN_SOLID needs to be defined for TYPE = 2, 3, 
4.    If  an  ALE  element  has  at  least  one  coupling  point  ,  this  element  will  be  selected  to  be  re-
fined (or removed).  The number of elements to refine is computed during the 
initialization.    NTOTRF  can  be  zero.    Otherwise  it  can  used  to  add  more  ele-
ments.  
3. 
4. 
If  NLVL = 1,  there  is  only  one  level  of  refinement:  the  ALE  elements  in  *ELE-
MENT_SOLID are the only ones to be replaced by clusters of 8 child elements.  
If  NLVL > 1,  there  are  several  levels  of  refinement:  not  only  the  initial  ALE 
elements in *ELEMENT_SOLID are refined but also their child elements.  
If only the 1st card is defined, a multi-material set id is not used.  It can be left to 
zero.  For the 2nd and 3rd cards, MMSID is the ID of *SET_MULTI-MATERIAL_-
GROUP_LIST in which the multi-material group ids (as defined in *ALE_MUL-
TI-MATERIAL_GROUP) are listed to select the ALE elements to be refined (or 
removed).    If  MMSID < 0,  only  mixed  ALE  elements  containing  all  the  multi-
material groups can be refined.  Otherwise clusters of 8 elements without a mix 
of the listed multi-material groups can be removed.  
5.  NTOTRF  defines  the  total  number  of  ALE  elements  to  be  refined.    So  for 
example NTOTRF = 100 with NLVL = 1 means that only 100 ALE elements can 
be replaced by 800 ALE finer elements (or 100 clusters of 8 child elements).  For 
NLVL = 2, these 800 elements can be replaced by 6400 finer elements.  
6. 
7. 
8. 
If  an  element  is  refined,  it  is  possible  to  refine  the  neighbor  elements  as  well.  
LAYRF  defines  the  number  of  neighbor  layers  to  refine.    For  example, 
LAYRF = 2  for  an  element  at  the  center  of  a  block  of  5 × 5 × 5  elements  will 
refine these 125 elements. 
If  MMSRM = 0,  MMSID  defines  the  multi-material  region  where  the  check  for 
refinement  removal  should  occur.    If  MMSRM  is  defined,  only  ALE  child  ele-
ments fully filled by the multi-material groups listed by the set MMSRM can be 
removed (if the refinement removal criterion is reached).  
If BEGRM < 0, the check for refinement removal is activated when the number 
of  8-element  clusters  for  the  refinement  is  below  a  limit  defined  by 
|BEGRM|*NTOTRF.  If |BEGRM| = 0.1, it means that the check for refinement 
removal starts when 90% of the stock of clusters is used for the refinement. 
9.  MAXRM < 0  defines  a  total  number  of  child  clusters  to  remove  for  the  whole 
run.  If positive, MAXRM defines an upper limit for the number of child clus-
ters to remove every NCYCRM cycles. 
10.  If  only  the  1st  card  is defined,  the  code  for  IELOUT  is  always  activated.   Since 
the  refinement  occurs  during  the  initialization,  every  refined  element  is  re-
placed by its 8 children in the set defined for *DATABASE_ELOUT.
11.  If there are more than 1 line, the code for IELOUT is activated if the flag is equal 
to  1.    Since  the  refinement  occurs  during  the  run,  the  parent  ids  in  the  set  de-
fined  for  *DATABASE_ELOUT  are  duplicated  8NLVL  times.    The  points  of  inte-
gration in the elout file are incremented to differentiate the child contributions 
to the database.
*CONTROL_REFINE_ALE2D 
Purpose:    Refine  ALE  quadrilateral  shell  elements  locally.    Each  parent  element  is 
replaced  by  4  child  elements  with  a  volume  equal  to  1/4th  the  parent  volume.   If  only 
the  1st  card  is  defined,  the  refinement  occurs  during  the  initialization.    The  2nd  card 
defines a criterion CRITRF to automatically refine the elements during the run.  If the 3rd 
card  is  defined,  the  refinement  can  be  removed  if  a  criterion  CRITRM  is  reached:  the 
child elements can be replaced by their parents. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
TYPE 
NLVL 
MMSID 
IBOX 
IELOUT 
Type 
I 
Default 
none 
I 
0 
I 
1 
I 
0 
I 
0 
I 
0 
Remaining cards are optional.† 
Automatic  refinement  card.    Optional  card  for  activating  automatic  refinement 
whereby  each  element  satisfying  certain  criteria  is  replaced  by  a  cluster  of  4  child 
elements 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NTOTRF  NCYCRF 
CRITRF 
VALRF 
BEGRF 
ENDRF 
LAYRF 
Type 
Default 
I 
0 
F 
0.0 
I 
0 
F 
F 
F 
0.0 
0.0 
0.0 
I
Automatic  Refinement  Remove  Card.    Optional  card  for  activating  automatic 
refinement removal whereby, when, for a cluster of 4 child elements, certain criteria are 
satisfied the clusters is replaced by its parent. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MAXRM  NCYCRM  CRITRM 
VALRM 
BEGRM 
ENDRM  MMSRM 
Type 
Default 
I 
0 
F 
0.0 
I 
0 
F 
F 
F 
0.0 
0.0 
0.0 
I 
0 
  VARIABLE   
DESCRIPTION
ID 
Set ID. 
TYPE 
Set type: 
EQ.0: ALE Part Set, 
EQ.1: ALE Part, 
EQ.2: Lagrangian Part Set coupled to ALE , 
EQ.3: Lagrangian Part coupled to ALE , 
EQ.4: Lagrangian Shell Set coupled to ALE , 
EQ.5: ALE Shell Set. 
NLVL 
Number of refinement levels .  
MMSID 
Multi-Material Set ID  : 
LT.0:  only  ALE  elements  with  all  the  multi-material  groups 
listed in *SET_MULTI-MATERIAL_GROUP_LIST can be 
refined (or removed otherwise) 
GT.0: ALE  elements  with  at  least  one  of  the  multi-material 
groups can be refined (or removed) 
IBOX 
Box  ID    defining  a  region  in  which  the  ALE 
elements are refined. 
IELOUT 
Flag to handle child data in elout .
VARIABLE   
DESCRIPTION
NTOTRF 
Total number of ALE elements to refine : 
GT.0:  Number of elements to refine 
EQ.0: NTOTRF = number  of  shell  elements  in  IBOX   
NCYCRF 
Number of cycles between each refinement. 
LT.0: |NCYCRF| is the time interval 
CRITRF 
Refinement criterion:  
EQ.0: static refinement (as if only the 1st card is defined), 
EQ.1: Pressure (if pressure > VALRF), 
EQ.2: Relative Volume (if V/Vo < VALRF)  , 
EQ.3: Volume Fraction (if Volume fraction > VALRF), 
EQ.5:  User defined criterion:  The 
routine  al2rfn_
criteria5  in  the  file  dynrfn_user.f  should  be  used  to  de-
velop  the  criterion.    The  file  is  part  of  the  general  pack-
age usermat.  
fortran 
VALRF 
Criterion value to reach for the refinement. 
BEGRF 
Time to begin the refinement. 
ENDRF 
Time to end the refinement. 
LAYRF 
Number of element layers to refine around a element reaching the
refinement criterion . 
MAXRM 
Maximum number of child clusters to remove : 
LT.0:  for the whole run, 
GT.0: every NCYCRM cycles 
NCYCRM 
Number of cycles between each check for refinement removal: 
LT.0: |NCYCRM| is the time interval
VARIABLE   
DESCRIPTION
CRITRM 
Criterion for refinement removal:  
EQ.0: no  refinement  removal  (as  if  only  the  1st  and  2nd  card 
are defined), 
EQ.1: Pressure (if pressure < VALRM), 
EQ.2: Relative Volume (if V/Vo > VALRM)  , 
EQ.3: Volume Fraction (if Volume fraction < VALRM), 
EQ.5:  User  defined  criterion:  The  fortran  routine  al2rmv_
criteria5 in the file dynrfn_user.f should be used to devel-
op  the  criterion.    The  file  is  part  of  the  general  package
usermat. 
VALRM 
Criterion  value  to  reach  in  each  child  element  of  a  cluster  for  its
removal (child elements of a cluster replaced by parent element). 
BEGRM 
Time to begin the check for refinement removal: 
LT.0: |BEGRM| represents a critical percent of NTOTRF below
which  the  check  for  refinement  removal  should  begin
(0.0 < |BEGRM| < 1.0).  . 
ENDRM 
Time to end the check for refinement removal. 
MMSRM 
Multi-Material Set ID for the refinement removal.   
Remarks: 
1. 
2. 
3. 
If only the 1st card is defined, only TYPE = 0,1,5 can be defined. 
*CONSTRAINED_LAGRANGE_IN_SOLID  needs 
for 
TYPE = 2,3,4.  If an ALE element has at least one coupling point , this element will be selected to be 
refined (or removed).     
be  defined 
to 
If  NLVL = 1,  there  is  only  one  level  of  refinement:  the  ALE  elements  in  *ELE-
MENT_SHELL are the only ones to be replaced by clusters of 4 child elements.  
If  NLVL > 1,  there  are  several  levels  of  refinement:  not  only  the  initial  ALE 
elements  in  *ELEMENT_SHELL  are  refined  but  also  their  child  elements.    If 
NLVL = 2 for example, the initial ALE elements can  be replaced by clusters of 
16 child elements. 
4. 
If only the 1st card is defined, a multi-material set id is not used.  It can be left to 
zero.  For the 2nd and 3rd cards, MMSID is the ID of *SET_MULTI-MATERIAL_-
GROUP_LIST in which the multi-material group ids (as defined in *ALE_MUL-
TI-MATERIAL_GROUP) are listed to select the ALE elements to be refined (or 
removed).    If  MMSID < 0,  only  mixed  ALE  elements  containing  all  the  multi-
material groups can be refined.  Otherwise clusters of 4 elements without a mix 
of the listed multi-material groups can be removed.  
5.  NTOTRF  defines  the  total  number  of  ALE  elements  to  be  refined.    So  for 
example NTOTRF = 100 means that only 100 ALE elements will be replaced by 
400  ALE  finer  elements  (or  100  clusters  of  4  child  elements).    For  NLVL = 2, 
these 400 elements can be replaced by 1600 finer elements. 
6. 
7. 
8. 
If  an  element  is  refined,  it  is  possible  to  refine  the  neighbor  elements  as  well.  
LAYRF  defines  the  number  of  neighbor  layers  to  refine.    For  example, 
LAYRF = 2 for an element at the center of a block of 5 × 5 elements will refine 
these 25 elements. 
If  MMSRM = 0,  MMSID  defines  the  multi-material  region  where  the  check  for 
refinement  removal  should  occur.    If  MMSRM  is  defined,  only  ALE  child  ele-
ments fully filled by the multi-material groups listed by the set MMSRM can be 
removed (if the refinement removal criterion is reached).  
If BEGRM < 0, the check for refinement removal is activated when the number 
of  4-element  clusters  for  the  refinement  is  below  a  limit  defined  by 
|BEGRM|*NTOTRF.  If |BEGRM| = 0.1, it means that the check for refinement 
removal starts when 90% of the stock of clusters is used for the refinement. 
9.  MAXRM < 0 is the exact opposite of NTOTRF > 0 and it defines a total number 
of child clusters to remove for the whole run.  If positive, MAXRM defines an 
upper limit for the number of child clusters to remove every NCYCRM cycles 
10.  If  only  the  1st  card  is defined,  the  code  for  IELOUT  is  always  activated.   Since 
the  refinement  occurs  during  the  initialization,  every  refined  element  is  re-
placed by its 4 children in the set defined for *DATABASE_ELOUT.  
11.  If there are more than 1 line, the code for IELOUT is activated if the flag is equal 
to  1.    Since  the  refinement  occurs  during  the  run,  the  parent  ids  in  the  set  de-
fined  for  *DATABASE_ELOUT  are  duplicated  4NLVL  times.    The  points  of  inte-
gration in the elout file are incremented to differentiate the child contributions 
to the database.
*CONTROL_REFINE_MPP_DISTRIBUTION 
Purpose:    Distribute  the  elements  for  the  refinement  over  the  MPP  processes.    This 
keyword addresses to the following situation:  
If  TYPE = 2,  3,  4  in  *CONTROL_REFINE_ALE,  the  refinement  occurs  around  a 
structure.    The  number  of  elements  for  this  refinement  is  computed  for  each 
process  according  the  initial  position  of  the  structure  in  each  MPP  subdomain 
(after the MPP decomposition of the ALE mesh during the phase 3 of the initiali-
zation, each process has a subdomain that is a portion of the ALE mesh).  If the 
structure is not in a subdomain, the related process receives no extra element for 
the refinement.  If the structure moves into this subdomain during the computa-
tion, the refinement around the structure can not occur.  To avoid this problem, 
the structure can be considered within a box (the structure maxima and minima 
give the box dimensions and positions).  This box moves and expands during the 
computation  to  keep  the  structure  inside.    An  estimation  of  the  maximal  dis-
placement and expansion will allow the code to evaluate which subdomains the 
structure  will  likely  cross  and  how  many  extra  elements  a  process  may  need to 
carry out the refinement. 
The computation of the number of extra elements per process occurs in 2 steps: 
•  If a file called “refine_mpp_distribution” does not exist in the working directory, 
it will be created to list the number of elements by process.  Each line in this file 
matches a process rank (starting from 0).  After the phase 3 of the MPP decompo-
sition,  the  run  terminates  as  if  *CONTROL_MPP_DECOMPOSITION_SHOW 
was activated. 
•  The model can be run again and the file “refine_mpp_distribution” will be read to 
allocate  the  memory  for  the  extra  elements  and  distribute  them  across  the  pro-
cesses. 
  Card 1 
Variable 
1 
ID 
Type 
I 
2 
DX 
F 
3 
DY 
F 
4 
DZ 
F 
5 
EX 
F 
6 
EY 
F 
7 
EZ 
F 
8 
Default 
none 
0.0 
0.0 
0.0 
1.0 
1.0 
1.0 
  VARIABLE   
DESCRIPTION
ID 
ID = -NTOTRF in *CONTROL_REFINE_ALE
VARIABLE   
DESCRIPTION
Dimensionless 𝑥-displacement of the box.  . 
Dimensionless 𝑦-displacement of the box.  . 
Dimensionless 𝑧-displacement of the box.  . 
Dimensionless 𝑥-expansion of the box.  . 
Dimensionless 𝑦-expansion of the box.  . 
Dimensionless 𝑧-expansion of the box.  . 
DX 
DY 
DZ 
EX 
EY 
EZ 
Remarks: 
1.  Box  Displacements.    DX,  DY  and  DZ  are  the  maximal  displacements  of  the 
box center.  These displacements are ratio of the box dimensions.  If, for exam-
ple, the largest length of the structure in the x-direction is 10m and the maximal 
displacement in this direction is 2m, DX should be equal to 0.2 
2.  Maximal  Box  Dilations.    EX,  EY  and  EZ  represent  the  maximal  dilatations  of 
the  box  in  each  direction.    These  expansions  are  ratio  of  the  box  dimensions.  
The box expands around its center.  If, for example, the maximal thickness of a 
structure along z is 1cm and the structure deforms 30 times the thickness in z-
direction, EZ should be equal to 30 and DZ=15 accounts for the box center mo-
tion.  The x-y plane is a plane of symmetry for this deformation, DZ can be zero.
*CONTROL 
Purpose:    Refine  quadrilateral  shell  elements  locally.    Each  parent  element  is  replaced 
by 4 child elements with a volume equal to 1/4th the parent volume.  If only the 1st card 
is  defined,  the  refinement  occurs  during  the  initialization.    The  2nd  card  defines  a 
criterion CRITRF to automatically refine the elements during the run.  If the 3rd card is 
defined,  the  refinement  can  be  removed  if  a  criterion  CRITRM  is  reached:  the  child 
elements can be replaced by their parents. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
TYPE 
NLVL 
IBOX 
IELOUT 
Type 
I 
Default 
none 
I 
0 
I 
1 
I 
0 
I 
0 
Remaining cards are optional.† 
Automatic  refinement  card.    Optional  card  for  activating  automatic  refinement 
whereby  each  element  satisfying  certain  criteria  is  replaced  by  a  cluster  of  4  child 
elements 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NTOTRF  NCYCRF 
CRITRF 
VALRF 
BEGRF 
ENDRF 
LAYRF 
Type 
Default 
I 
0 
F 
0.0 
I 
0 
F 
F 
F 
0.0 
0.0 
0.0 
I
Automatic  Refinement  Remove  Card.    Optional  card  for  activating  automatic 
refinement removal whereby, when, for a cluster of 4 child elements, certain criteria are 
satisfied the clusters is replaced by its parent. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MAXRM  NCYCRM  CRITRM 
VALRM 
BEGRM 
ENDRM 
Type 
Default 
I 
0 
F 
0.0 
I 
0 
F 
F 
F 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
ID 
Set ID. 
LT.0: parent  elements  can  be  hidden  in  lsprepost  as  they  are
replaced by their children. 
TYPE 
Set type:: 
EQ.0: Part Set, 
EQ.1: Part, 
EQ.2: Shell Set. 
NLVL 
IBOX 
Number of refinement levels .  
Box  ID    defining  a  region  in  which  the 
elements are refined. 
IELOUT 
Flag to handle child data in the elout file .  
NTOTRF 
Total number of elements to refine : 
GT.0:  Number of elements to refine 
EQ.0: NTOTRF = number of shell elements in IBOX 
NCYCRF 
Number of cycles between each refinement. 
LT.0: |NCYCRF| is the time interval
VARIABLE   
DESCRIPTION
CRITRF 
Refinement criterion:  
EQ.0: static refinement (as if only the 1st card is defined), 
EQ.1: Pressure (if pressure > VALRF), 
EQ.2: undefined , 
EQ.3: Von Mises criterion, 
EQ.4: Criterion similar to ADPOPT = 4 in *CONTROL_ADAP-
TIVE (VALRF = ADPTOL), 
EQ.5:  User defined criterion:  The 
routine  shlrfn_
criteria5 in the file dynrfn_user.f should be used to devel-
op  the  criterion.    The  file  is  part  of  the  general  package
usermat. 
fortran 
VALRF 
Criterion value to reach for the refinement. 
BEGRF 
Time to begin the refinement. 
ENDRF 
Time to end the refinement. 
LAYRF 
Number of element layers to refine around a element reaching the
refinement criterion . 
MAXRM 
Maximum number of child clusters to remove : 
LT.0:  for the whole run, 
GT.0: every NCYCRM cycles 
NCYCRM 
Number of cycles between each check for refinement removal: 
LT.0: |NCYCRM| is the time interval
VARIABLE   
DESCRIPTION
CRITRM 
Criterion for refinement removal:  
EQ.0: no  refinement  removal  (as  if  only  the  1st  and  2nd  card
are defined), 
EQ.1: Pressure (if pressure < VALRM), 
EQ.2: undefined, 
EQ.3: Von Mises criterion, 
EQ.4: Criterion similar to ADPOPT = 4 in *CONTROL_ADAP-
TIVE (VALRF = ADPTOL), 
EQ.5:  User defined criterion:  The  fortran  routine  shlrmv_
criteria5  in  the  file  dynrfn_user.f  should  be  used  to  de-
velop  the  criterion.    The  file  is  part  of  the  general  pack-
age usermat. 
VALRM 
Criterion value to reach in each child elements of a cluster for its
removal (child elements replaced by parent element). 
BEGRM 
Time to begin the check for refinement removal. 
LT.0: |BEGRM| represents a critical percent of NTOTRF below
which  the  check  for  refinement  removal  should  begin
(0.0 < |BEGRM| < 1.0).  . 
ENDRM 
Time to end the check for refinement removal. 
Remarks: 
1. 
If NLVL = 1, there is only one level of refinement: the elements in *ELEMENT_-
SHELL  are  the  only  ones  to  be  replaced  by  clusters  of  4  child  elements.    If 
NLVL > 1, there are several levels of refinement: not only the initial elements in 
*ELEMENT_SHELL  are  refined  but  also  their  child  elements.    If  NLVL = 2  for 
example, the initial elements can be replaced by clusters of 16 child elements. 
2.  NTOTRF  defines  the  total  number  of  elements  to  be  refined.    So  for  example 
NTOTRF = 100 with NLVL = 1 means that only 100 elements can be replaced by 
400 finer elements (or 100 clusters of 4 child elements).  For NLVL = 2, these 400 
elements can be replaced by 1600 finer elements.  
3. 
If  an  element  is  refined,  it  is  possible  to  refine  the  neighbor  elements  as  well.  
LAYRF  defines  the  number  of  neighbor  layers  to  refine.    For  example, 
LAYRF = 2 for an element at the center of a block of 5 × 5 elements will refine 
these 25 elements.
4. 
If BEGRM < 0, the check for refinement removal is activated when the number 
of 4-element clusters for the refinement is below a limit defined by |BEGRM| × 
NTOTRF.    If  |BEGRM| = 0.1,  it  means  that  the  check  for  refinement  removal 
starts when 90% of the stock of clusters is used for the refinement. 
5.  MAXRM < 0  defines  a  total  number  of  child  clusters  to  remove  for  the  whole 
run.  If positive, MAXRM defines an upper limit for the number of child clus-
ters to remove every NCYCRM cycles. 
6. 
7. 
If  only  the  1st  card  is defined,  the  code  for  IELOUT  is  always  activated.   Since 
the  refinement  occurs  during  the  initialization,  every  refined  element  is  re-
placed by its 4 children in the set defined for *DATABASE_ELOUT.  
If there are more than 1 line, the code for IELOUT is activated if the flag is equal 
to  1.    Since  the  refinement  occurs  during  the  run,  the  parent  ids  in  the  set  de-
fined  for  *DATABASE_ELOUT  are  duplicated  4NLVL  times.    The  points  of  inte-
gration in the elout file are incremented to differentiate the child contributions 
to the database.
*CONTROL_REFINE_SOLID 
Purpose:  Refine hexahedral solid elements locally.  Each parent element is replaced by 
8 child elements with a volume equal to 1/8th the parent volume.  If only the 1st card is 
defined, the refinement occurs during the initialization.  The 2nd card defines a criterion 
CRITRF to automatically refine the elements during the run.  If the 3rd card is defined, 
the refinement can be removed if a criterion CRITRM is reached: the child elements can 
be replaced by their parents. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
TYPE 
NLVL 
IBOX 
IELOUT 
Type 
I 
Default 
none 
I 
0 
I 
1 
I 
0 
I 
0 
Remaining cards are optional.† 
Automatic  refinement  card.    Optional  card  for  activating  automatic  refinement 
whereby  each  element  satisfying  certain  criteria  is  replaced  by  a  cluster  of  8  child 
elements 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NTOTRF  NCYCRF 
CRITRF 
VALRF 
BEGRF 
ENDRF 
LAYRF 
Type 
Default 
I 
0 
F 
0.0 
I 
0 
F 
F 
F 
0.0 
0.0 
0.0 
I
Automatic  Refinement  Remove  Card.    Optional  card  for  activating  automatic 
refinement removal whereby, when, for a cluster of 8 child elements, certain criteria are 
satisfied the clusters is replaced by its parent. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MAXRM  NCYCRM  CRITRM 
VALRM 
BEGRM 
ENDRM 
Type 
Default 
I 
0 
F 
0.0 
I 
0 
F 
F 
F 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
ID 
Set ID. 
LT.0: parent  elements  can  be  hidden  in  lsprepost  as  they  are
replaced by their children. 
TYPE 
Set type: 
EQ.0: Part Set, 
EQ.1: Part, 
EQ.2: Solid Set. 
NLVL 
IBOX 
Number of refinement levels.  See Remark 1.  
Box  ID    defining  a  region  in  which  the 
elements are refined. 
IELOUT 
Flag to handle child data in elout.  See Remarks 6 and 7.  
NTOTRF 
Total number of elements to refine.  See Remark 2. 
GT.0:  Number of elements to refine 
EQ.0: NTOTRF = number of solid elements in IBOX 
NCYCRF 
Number of cycles between each refinement. 
LT.0: |NCYCRF| is the time interval
VARIABLE   
DESCRIPTION
CRITRF 
Refinement criterion:  
EQ.0: static refinement as if only the 1st card is defined, 
EQ.1: Pressure, if pressure > VALRF, 
EQ.2: undefined , 
EQ.3: Von Mises criterion. 
EQ.5:  User  defined  criterion.    The  fortran  routine  sldrfn_
criteria5 in the file dynrfn_user.f should be used to devel-
op  the  criterion.    The  file  is  part  of  the  general  package
usermat. 
VALRF 
Criterion value to reach for the refinement. 
BEGRF 
Time to begin the refinement. 
ENDRF 
Time to end the refinement. 
LAYRF 
Number  of  element  layers  to  refine  around  an  element  reaching
the refinement criterion.  See Remark 3. 
MAXRM 
Maximum number of child clusters to remove.  See Remark 5. 
LT.0:  for the whole run, 
GT.0: every NCYCRM cycles 
NCYCRM 
Number of cycles between each check for refinement removal: 
LT.0: |NCYCRM| is the time interval 
CRITRM 
Criterion for removal of refinement:  
EQ.0: no removal of refinement as if only the 1st and 2nd card
are defined, 
EQ.1: Pressure if pressure < VALRM, 
EQ.2: undefined, 
EQ.3: Von Mises criterion. 
EQ.5:  User  defined  criterion.    The  FORTRAN  routine  sldrmv_
criteria5 in the file dynrfn_user.f should be used to devel-
op  the  criterion.    The  file  is  part  of  the  general  package
usermat.
VARIABLE   
VALRM 
DESCRIPTION
Criterion  value  to  reach  in  each  child  element  of  a  cluster  for  its
removal (replace child elements with parent element). 
BEGRM 
Time to begin check for refinement removal: 
LT.0: |BEGRM| represents a critical percent of NTOTRF below
which  the  check  for  refinement  removal  should  begin
(0.0 < |BEGRM| < 1.0).  See Remark 4. 
ENDRM 
Time to end the check for refinement removal. 
Remarks: 
1.  Number  of  Refinement  Levels.    If  NLVL=1,  there  is  only  one  level  of 
refinement: the elements in *ELEMENT_SOLID are the only ones to be replaced 
by clusters of 8 child  elements.  If NLVL > 1, there are several levels of refine-
ment:  not  only  the  initial  elements  in  *ELEMENT_SOLID  are  refined  but  also 
their  child  elements.    If  NLVL = 2  for  example,  the  initial  elements  can  be  re-
placed by clusters of 64 child elements. 
2.  Maximum Number of Elements to Refine.  NTOTRF defines the total number 
of  elements  to  be  refined.    So  for  example  NTOTRF=100  with  NLVL=1  means 
that only 100 elements can be replaced by 800 finer elements (or 100 clusters of 
8  child  elements).    For  NLVL=2,  these  800  elements  can  be  replaced  by  6400 
finer elements.  
3.  Number  of  Layers  to  Refine.    If  an  element  is  refined,  it  is  possible  to  refine 
the neighbor elements as well.  LAYRF defines the number of neighbor layers to 
refine.    For  example,  LAYRF=2  for  an  element  at  the  center  of  a  block  of 
5 × 5 × 5 elements will refine these 125 elements. 
4.  Onset  of  Refinement  Removal.    If  BEGRM < 0,  the  check  for  refinement 
removal is activated when the number of 8-element clusters for the refinement 
is below a limit defined by |BEGRM| × NTOTRF.  If |BEGRM| = 0.1, it means 
that the check for refinement removal starts when 90% of the  stock of clusters 
are used for the refinement. 
5.  Maximum Refinement Removal.  MAXRM < 0 defines a total number of child 
clusters  to  remove  for  the  whole  run.    If  positive,  MAXRM  defines  an  upper 
limit for the number of child clusters to remove every NCYCRM cycles. 
6.  The “elout” Database and Initial Refinement.  If only the 1st card is defined, 
the  code  for  IELOUT  is  always  activated.    Since  the  refinement  occurs  during
the  initialization,  every  refined  element  is  replaced  by  its  8  children  in  the  set 
defined for *DATABASE_ELOUT.  
7.  The “elout” Database and Refinement at Run Time.  If there are more than 1 
line, the code for IELOUT is activated if the flag is equal to 1.  Since the refine-
ment occurs during the run, the parent ids in the set defined for *DATABASE_-
ELOUT  are  duplicated  8NLVL  times.    The  points  of  integration  in  the  elout  file 
are incremented to differentiate the child contributions to the database.
*CONTROL_REMESHING_{OPTION} 
Available options include: 
<BLANK> 
EFG 
Purpose:  Provide control over the remeshing of solids which are meshed with the solid 
tetrahedron  element  type  13  and  mesh-free  solid  types  41,  42.    The  element  size  for 
three-dimensional  adaptivity  can  be  set  on  the  surface  mesh  of  the  solid  part,  and 
adaptivity  can  be  activated  based  on  the  criteria  of  volume  loss,  mass  increase,  or 
minimum  time  step  size.    In  addition,  so-called  interactive  adaptivity  triggers  can  be 
invoked using the EFG option. 
There are two types of 3-D solid adaptivity affected by *CONTROL_REMESHING:  
1.  General  tetrahedral  adaptivity  for  which  the  EFG  option  of  *CONTROL_-
REMESHING may be invoked.  See ADPOPT = 2 in *PART. 
2.  Axisymmetric  adaptivity,  sometimes  called  orbital  adaptivity,  in  which 
remeshing  is  done  with  hexahedral  and  pentahedral  elements.    See  AD-
POPT = 3  in  *PART.    The  EFG  option  of  *CONTROL_REMESHING  does  not 
apply for this type of adaptivity. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RMIN 
RMAX 
VF_LOSS MFRAC 
DT_MIN 
ICURV 
CID 
SEGANG 
Type 
F 
F 
F 
F 
Default 
none 
none 
1.0 
0.0 
F 
0. 
I 
4 
I 
0 
F 
0.0 
Additional card for EFG option. 
  Card 2 
1 
Variable 
IVT 
Type 
Default 
I 
1 
LS-DYNA R10.0 
2 
IAT 
I 
0 
3 
4 
5 
6 
7 
8 
IAAT 
IER 
MM 
I 
0 
I 
0
Second additional card for EFG option.  This card is optional. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IAT1 
IAT2 
IAT3 
Type 
F 
F 
F 
Default 
1020 
1020 
1020 
  VARIABLE   
DESCRIPTION
RMIN 
RMAX 
VF_LOSS 
MFRAC 
DT_MIN 
Minimum edge length for the surface mesh surrounding the parts
which should be remeshed. 
Maximum edge length for the surface mesh surrounding the parts 
which should be remeshed. 
Volume fraction loss required in a type 13 tetrahedral elements to
trigger a remesh.  In the type 13 solid elements, the pressures are
computed at the nodal points; therefore, it is possible for volume 
to  be  conserved  but  for  individual  tetrahedrons  to  experience  a
significant  volume  loss  or  gain.    The  volume  loss  can  lead  to
numerical  problems.    Recommended  values  for  VF_LOSS  in  the 
range of 0.10 to 0.30 may be reasonable. 
Mass  ratio  gain  during  mass  scaling  required  for  triggering  a 
remesh.    For  a  one  percent  increase  in  mass,  set  MFAC = 0.010. 
This  variable  applies  to  both  to  general  three  dimensional
tetrahedral  remeshing  and  to  three  dimensional  axisymmetric
remeshing. 
Time  step  size  required  for  triggering  a  remesh.      This  option
applies  only  to  general  three  dimensional  tetrahedral  remeshing
and  is  checked  before  mass  scaling  is  applied  and  the  time  step
size reset.   
ICURV 
Define number of element along the radius in the adaptivity.  See 
remark 3.
VARIABLE   
CID 
DESCRIPTION
Coordinate  system  ID  for  three  dimensional  axisymmetric
remeshing.    The  z-axis  in  the  defined  coordinate  system  is  the 
orbital  axis,  and  has  to  be  parallel  to  the  global  z-axis  in  the 
current axisymmetric remesher. 
EQ.0: use global coordinate, and the global 𝑧-axis is the orbital 
axis (default) 
SEGANG 
  For Axisymmetric 3-D remeshing:  Angular 
element 
size 
  For General (tet) 3-D remeshing:  Critical  angle  specified 
in 
radians  to  preserve  feature 
lines. 
(degrees). 
IVT 
Internal variable transfer in adaptive EFG. 
EQ.1:  Moving  Least  square  approximation  with  Kronecker-
delta property (recommended in general case). 
EQ.-1:  Moving 
square 
Least 
Kronecker-delta property. 
approximation  without
EQ.2:  Partition  of  unity  approximation  with  Kronecker-delta 
property. 
EQ.-2:  Partition  of  unity  approximation  without  Kronecker-
delta property.  
EQ.-3:  Finite element approximation. 
IAT 
Flag for interactive adaptivity. 
EQ.0:  No interactive adaptivity. 
EQ.1:  Interactive  adaptivity 
combined  with  predefined 
adaptivity. 
EQ.2:  Purely interactive adaptivity.  The time interval between
two successive adaptive steps is bounded by ADPFREQ.
EQ.3:  Purely interactive adaptivity. 
IAAT 
Interactive adaptivity adjustable tolerance. 
EQ.0: The  tolerance  to  trigger  interactive  adaptivity  is  not 
adjusted. 
EQ.1: The  tolerance  is  adjusted  in  run-time  to  avoid  over-
activation.
IER 
*CONTROL_REMESHING 
DESCRIPTION
Interactive  adaptive  remeshing  with  element  erosion  for  metal
cutting. 
EQ.1: The failed elements are eroded and the cutting surface is
reconstructed  before  adaptive  remeshing.    The  current
implementation only supports SMP and IAT = 1, 2, 3. 
MM 
Interactive adaptive remeshing with monotonic resizing. 
EQ.1: The  adaptive  remeshing  can  not  coarsen  a  mesh.    The 
current  implementation  only  supports  IAT = 1,  2,  3  and 
IER = 0. 
Shear  strain  tolerance  for  interactive  adaptivity.    If  the  shear
strain in any 
formulation 42 EFG tetrahedral element exceeds IAT1, remeshing
is triggered.  (0.1 ~ 0.5 is recommended). 
𝐿max/𝐿min   tolerance  where  𝐿max  and  𝐿min  are  the  maximum  and 
minimum  edge  lengths  of    any  given  formulation  42  EFG
tetrahedral  element.    If  this  ratio  in  any  element  exceeds  IAT2,
remeshing is triggered.  (RMAX/RMIN is recommended.) 
Volume change tolerance.  If the normalized change in volume of
any  formulation  42  tetrahedral  element,  defined  as  ∣𝑣1 − 𝑣0∣/∣𝑣0∣
where  𝑣1  is  the  current  element  volume  and  𝑣0   is  the  element 
volume  immediately  after  the  most  recent  remeshing,  exceeds 
IAT3, remeshing is triggered.  (0.5 is recommended.) 
IAT1 
IAT2 
IAT3 
Remarks: 
1.  The  value  of  RMIN  and  RMAX  should  be  of  the  same  order.    The  value  of 
RMAX can be set to 2-5 times greater than RMIN. 
2.  When interactive adaptivity is invoked (IAT > 0), even if none of the tolerances 
IAT1,  IAT2,  and  IAT3  for  the  three  respective  indicators  (shear  strain,  edge 
length  ratio,  normalized  volume  change)  are  exceeded,  remeshing  will  still  be 
triggered if any of the three indicators over a single explicit time step changes 
by more than 50%, that is, if 
|[value]𝑛 − [value]𝑛−1|
|[value]𝑛−1|
> 0.5
where  [value]𝑛  denotes  value  of  indicator  in  nth  (current)  time  step  and 
[value]𝑛−1 denotes value of indicator in previous time step .  This condition is 
checked only if [value]𝑛−1 is nonzero. 
3. 
ICURV represents a number of elements and applies only when ADPENE > 0 in 
*CONTROL_ADAPTIVE.    The  “desired  element  size”  at  each  point  on  slave 
contact  surface  is  computed  based  on  the  tooling  radius  of  curvature  ,  so  that  ICURV  elements 
would  be  used  to  resolve  a  hypothetical  90  degree  arc  at  the  tooling  radius  of 
curvature.  The value of ICURV is (internally) limited to be >=2 and <=12.  The 
final adapted element size is adjusted as necessary to fall within the size range 
set forth by RMIN and RMAX.
*CONTROL_REQUIRE_REVISION 
Purpose:    To  prevent  the  model  from  being  run  in  old  versions  of  LS-DYNA.    This 
might  be  desirable  due  to  known  improvements  in  the  program,  required  capability, 
etc. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  RELEASE  REVISION 
Type 
C 
I 
Default 
none 
none 
  VARIABLE   
RELEASE 
DESCRIPTION
The  release  of  code  required.    This  should  be  a  string  such  as
“R6.1.0” or “R7.0” 
REVISION 
The  minimum  revision  required.    This  corresponds  to  the  “SVN
Version” field in the d3hsp file.   
Remarks: 
1.  Any  number  of  lines  can  appear,  indicating  for  example  that  a  particular 
feature was introduced in different release branches at different times. 
2. 
If  the  RELEASE  field  is  left  empty,  then  any  executable  whose  development 
split from the main SVN trunk after the given REVISION will be allowed. 
Example: 
*CONTROL_REQUIRE_REVISION 
R6.1    79315 
R7.0    78310 
        78304 
This  would  prevent  execution  by  any  R6.1  executable  before  r79315,  any  R7.0  before 
r78310, and all other executables whose development split from the main trunk before 
r78304.    Note  that  no  versions  of  R6.0,  R6.0.0,  or  R6.1.0  are  allowed:  R6.1  does  NOT 
imply R6.1.0, no matter what the revision of R6.1.0 – R6.1.0 would have to be explicitly 
listed.  Similarly, R7.0.0 would not be allowed because it is not listed, and it split from
the trunk in r76398.   Any future R8.X executable would be allowed, since it will have 
split from the trunk after r78304.
*CONTROL_RIGID 
Purpose:    Special  control  options  related  to  rigid  bodies  and  to  linearized  flexible 
bodies, see *PART_MODES. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LMF 
JNTF 
ORTHMD
PARTM 
SPARSE  METALF 
PLOTEL 
RBSMS 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
Remaining cards are optional.† 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NORBIC 
Type 
Default 
I 
0 
  VARIABLE   
LMF 
DESCRIPTION
Switch  the  explicit  rigid  body  joint  treatment  to  an  implicit
impose
formulation  which  uses  Lagrange  multipliers 
prescribed  kinematic  boundary  conditions  and  joint  constraints.
There  is  a  slight  cost  overhead  due  to  the  assembly  of  sparse
matrix equations which are solved using standard procedures for
nonlinear  problems  in  rigid  multi-body  dynamics.    Lagrange 
multiplier flag: 
to 
EQ.0: explicit penalty formulation 
EQ.1: implicit formulation with Lagrange multipliers
VARIABLE   
DESCRIPTION
JNTF 
Generalized joint stiffness formulation; see Remark 1 below: 
EQ.0: incremental update 
EQ.1: total formulation (exact) 
EQ.2:  total formulation intended for implicit analysis 
ORTHMD 
Orthogonalize modes with respect to each other: 
EQ.0: true 
EQ.1: false, the modes are already orthogonalized 
PARTM 
Use global mass matrix to determine part mass distribution.  This
mass matrix may contain mass from other parts that share nodes.
See Remark 2 below. 
EQ.0: true 
EQ.1: false 
SPARSE 
Use  sparse  matrix  multiply  subroutines  for  the  modal  stiffness
and damping matrices.  See Remark 3. 
EQ.0: false, do full matrix multiplies (frequently faster). 
EQ.1: true 
MATELF 
Metal  forming  option,  which  should  not  be  used  for  crash  and
other applications involving rigid bodies.  Use fast update of rigid
body  nodes.    If  this  option  is  active  the  rotational  motion  of  all
rigid bodies should be suppressed. 
EQ.0: full treatment is used 
EQ.1: fast update for metal forming applications 
PLOTEL 
Automatic  generation  of  *ELEMENT_PLOTEL 
STRAINED_NODAL_RIGID_BODY.  
for  *CON-
EQ.0: no generation 
EQ.1: one  part  is  generated for  all  nodal  rigid  bodies  with  the
PID set to 1000000. 
EQ.2: one  part  is  generated  for  each  nodal  rigid  body  in  the
problem  with  a  part  ID  of  1000000 + PID,  where  PID  is 
the nodal rigid body ID.
RBSMS 
*CONTROL_RIGID 
DESCRIPTION
Flag to apply consistent treatment of rigid bodies in selective and
conventional mass scaling, Remark 4. 
EQ.0: Off 
EQ.1: On 
NORBIC 
Circumvent rigid body inertia check, see Remark 5.  
EQ.0: Off 
EQ.1: On 
Remarks: 
1.  JNTF.    The  default  behavior  is  for  the  relative  angles  between  the  two 
coordinate  systems  to  be  done  incrementally.    This  is  an  approximation,  in 
contrast to the total formulation where the angular offsets are computed exact-
ly.  The disadvantage of the latter approach is that a singularity exists when an 
offset  angle  equals  180  degrees.    In  most  applications,  the  stop  angles  exclude 
this possibility and JNTF=1 should not cause a problem.  JNTF=2 is implement-
ed with smooth response and especially intended for implicit analysis. 
2.  PARTM.    If  the  determination  of  the  normal  modes  included  the  mass  from 
both connected bodies and discrete masses, or if there are no connected bodies, 
then  the  default  is  preferred.    When  the  mass  of  a  given  part  ID  is  computed, 
the resulting mass vector includes the mass of all rigid bodies that are merged 
to the given part ID, but does not included discrete masses.  See the keyword: 
*CONSTRAINED_RIGID_BODIES.  A lumped mass matrix is always assumed. 
3.  SPARSE.  Sparse matrix multipliers save a substantial number of operations if 
the matrix is truly sparse.  However, the overhead will slow the multipliers for 
densely populated matrices. 
4.  RBSMS.    In  selective  mass  scaling,  rigid  bodies  connected  to  deformable 
elements  can  result  in  significant  addition  of  inertia  due  missing  terms  in  the 
SMS mass matrix.  This problem has been observed in automotive applications 
where spotwelds are modeled using constrained nodal rigid bodies.  By apply-
ing  consistent  rigid  body  treatment  significant  improvement  in  accuracy  and 
robustness  are  observed  at  the  expense  of  increased  CPU  intensity.    This  flag 
also applies to conventional mass scaling as it has been observed that inconsist-
encies for various reasons may result in unstable solution schemes even for this 
case.
5.  NORBIC. During initialization, the determinant of the rigid body inertia tensor 
is checked.  If it falls below a tolerance value of 10−30, LS-DYNA issues an error 
message  and  the  calculation  stops.    In  some  rare  cases  (e.g.    with  an  adverse 
system  of  units),  such  tiny  values  would  still  be  valid.    In  this  case,  NORBIC 
should be set to 1 to circumvent the implied inertia check.
*CONTROL_SHELL 
Purpose:  Provide controls for computing shell response. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  WRPANG 
ESORT 
IRNXX 
ISTUPD 
THEORY 
BWC 
MITER 
PROJ 
Type 
F 
Default 
20. 
I 
0 
I 
-1 
I 
0 
I 
2 
I 
2 
I 
1 
I 
0 
Remaining cards are optional.† 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  ROTASCL 
INTGRD 
LAMSHT  CSTYP6 
THSHEL 
Type 
F 
Default 
1. 
  Card 3 
1 
I 
0 
2 
I 
0 
3 
I 
1 
4 
I 
0 
5 
6 
7 
8 
Variable 
PSTUPD  SIDT4TU 
CNTCO 
ITSFLG 
IRQUAD  W-MODE  STRETCH 
ICRQ 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
F 
F 
I 
0 
inactive 
inactive
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NFAIL1 
NFAIL4 
PSNFAIL 
KEEPCS 
DELFR 
DRCPSID  DRCPRM 
INTPERR 
Type 
I 
I 
I 
Default 
inactive 
inactive 
0 
I 
0 
I 
0 
I 
0 
F 
1.0 
  VARIABLE   
WRPANG 
DESCRIPTION
Shell  element  warpage  angle  in  degrees.    If  a  warpage  greater
than this angle is found, a warning message is printed.  Default is
20 degrees. 
ESORT 
Sorting  of  triangular  shell  elements  to  automatically  switch
degenerate  quadrilateral  shell  formulations  to  more  suitable 
triangular shell formulations. 
EQ.0: Do not sort (default). 
EQ.1: Sort  (switch  to  C0  triangular  shell  formulation  4,  or  if  a
quadratic  shell,  switch  to  shell  formulation  24,  or  if  a
shell  formulation  with  thickness  stretch,  switch  to  shell
formulation 27). 
EQ.2: Sort (switch to DKT triangular shell formulation 17, or if
a  quadratic  shell,  switch  to  shell  formulation  24).    The
DKT  formulation  will  be  unstable  if  used  to  model  an
uncommonly thick, triangular shell. 
IRNXX 
Shell normal update option.  This option affects the Hughes-Liu, 
Belytschko-Wong-Chiang, 
shell 
formulations  (including  fully  integrated  shells  -16  and  16).    The 
latter  is  affected  if  and  only  if  the  warping  stiffness  option  is
active, i.e., BWC = 1. 
the  Belytschko-Tsay 
and 
EQ.-2:  unique  nodal  fibers  which  are  incrementally  updated
based on the nodal rotation at the location of the fiber, 
EQ.-1:  recomputed fiber directions each cycle, 
EQ.0:  default set to -1, 
EQ.1:  compute on restarts, 
EQ.n:  compute every n cycles (Hughes-Liu shells only).
ISTUPD 
*CONTROL_SHELL 
DESCRIPTION
Shell  thickness  change  option  for  deformable  shells. 
  The
parameter,  PSTUPD,  on  the  second  optional  card  allows  this
option to be applied by part ID.  For crash analysis, neglecting the
elastic  component  of  the  strains,  ISTUPD = 4,  may  improve 
energy conservation and stability. 
EQ.0: no thickness change. 
EQ.1: membrane  straining  causes  thickness  change  in  3  and  4
node  shell  elements.    This  option  is  very  important  in
sheet metal forming or whenever membrane stretching is 
important. 
EQ.2: membrane  straining  causes  thickness  change  in  8  node
thick  shell  elements,  types  1  and  2.    This  option  is  not
recommended for implicit or explicit solutions which use
the fully integrated type 2 elements.  Types 3 and 5 thick
shells  are  continuum  based  and  thickness  changes  are
always considered. 
EQ.3: options 1 and 2 apply. 
EQ.4: option  1  applies,  but  the  elastic  strains  are  neglected  for
the  thickness  update.    This  option  only  applies  to  shells
(not  thick  shells)  and  the  most  common  elastic-plastic 
materials for which the elastic response is isotropic.  See
SIDT4TU for selective application of this option. 
THEORY 
list  of  shell
Default  shell  formulation. 
  For  remarks  on 
formulations,  refer  to  *SECTION_SHELL. 
overriding  this  default  and  how  THEORY  may  affect  contact 
behavior, see Remark 2. 
  For  a  complete 
EQ.1:  Hughes-Liu 
EQ.2:  Belytschko-Tsay (default) 
EQ.3:  BCIZ triangular shell (not recommended) 
EQ.4:  C0 triangular shell 
EQ.5:  Belytschko-Tsay membrane 
EQ.6:  S/R Hughes Liu 
EQ.7:  S/R co-rotational Hughes Liu 
EQ.8:  Belytschko-Leviathan shell 
EQ.9:  fully integrated Belytschko-Tsay membrane
VARIABLE   
DESCRIPTION
EQ.10:  Belytschko-Wong-Chiang 
EQ.11:  Fast (co-rotational) Hughes-Liu 
EQ.12:  Plane stress (𝑥-𝑦 plane) 
EQ.13:  Plane strain (𝑥-𝑦 plane) 
EQ.14:  Axisymmetric  solid  (𝑦-axis  of  symmetry)  –  area 
weighted.  See Remark 5 
EQ.15:  Axisymmetric  solid  (𝑦-axis  of  symmetry)  –  volume 
weighted.  See Remark 5 
EQ.16:  Fully integrated shell element (very fast) 
EQ.17:  Discrete Kirchhoff triangular shell (DKT) 
EQ.18:  Discrete  Kirchhoff  linear  shell  either  quadrilateral  or 
Triangular with 6DOF per node 
EQ.20:  C0 linear shell element with 6 DOF per node 
EQ.21:  C0  linear  shell  element  with  5  DOF  per  node  with  the
Pian-Sumihara  membrane  hybrid  quadrilateral  mem-
brane 
EQ.25:  Belytschko-Tsay shell with thickness stretch 
EQ.26:  Fully integrated shell with thickness stretch 
EQ.27:  C0 triangular shell with thickness stretch 
BWC 
Warping stiffness for Belytschko-Tsay shells: 
EQ.1:  Belytschko-Wong-Chiang warping stiffness added.   
EQ.2: Belytschko-Tsay (default). 
MITER 
Plane  stress  plasticity  option  (applies  to  materials  3,  18,  19,  and
24): 
EQ.1: iterative plasticity with 3 secant iterations (default), 
EQ.2: full iterative plasticity, 
EQ.3: radial  return  noniterative  plasticity.    May  lead  to  false
results and has to be used with great care.   
PROJ 
Projection  method  for  the  warping  stiffness  in  the  Belytschko-
Tsay  shell  (the  BWC  option  above)  and  the  Belytschko-Wong-
Chiang elements .  This parameter applies to 
explicit  calculations  since  the  full  projection  method  is  always 
used  if  the  solution  is  implicit  and  this  input  parameter  is
VARIABLE   
DESCRIPTION
ignored. 
EQ.0: drill projection, 
EQ.1: full projection. 
ROTASCL 
Define a scale factor for the rotary shell mass.  This option is not
for  general  use.    The  rotary  inertia  for  shells  is  automatically
scaled to permit a larger time step size.  A scale factor other than
the default, i.e., unity, is not recommended. 
INTGRD 
Default  through  thickness  numerical  integration  rule  for  shells
and thick shells.  If more than 10 integration points are requested,
a trapezoidal rule is used unless a user defined rule is specified. 
EQ.0: Gauss integration: If 1-10 integration points are specified, 
the default rule is Gauss integration. 
EQ.1: Lobatto integration: 
If  3-10  integration  points  are 
specified, the default rule is Lobatto.  For 2 point integra-
tion,  the  Lobatto  rule  is  very  inaccurate,  so  Gauss  inte-
gration  is  used  instead.    Lobatto  integration  has  an 
advantage  in  that  the inner and  outer  integration  points
are on the shell surfaces. 
LAMSHT 
Laminated  shell  theory  flag.    Except  for  those  using  the  Green-
Lagrange strain tensor, laminated  shell theory is available  for all
thin  shell  and  thick  shell  materials.    It  is  activated  when
LAMSHT =  3,  4, or 5  and  by  using  *PART_COMPOSITE  or  *IN-
TEGRATION_SHELL  to  define  the 
  See
Remark 6. 
integration  rule. 
EQ.0: do not update shear corrections, 
EQ.1: activate laminated shell theory, 
EQ.3: activate laminated thin shells, 
EQ.4: activate laminated shell theory for thick shells, 
EQ.5: activate laminated shell theory for thin and thick shells. 
Coordinate  system  for  the  type  6  shell  element.    The  default 
system  computes  a  unique  local  system  at  each  in  plane  point.
just  one  system  used
The  uniform  local  system  computes 
throughout  the  shell  element.    This  involves  fewer  calculations
and is therefore more efficient.  The change of systems has a slight 
effect  on  results;  therefore,  the  older,  less  efficient  method  is  the
CSTYP6
VARIABLE   
DESCRIPTION
THSHEL 
PSTUPD 
SIDT4TU 
CNTCO 
default. 
EQ.1: variable local coordinate system (default), 
EQ.2: uniform local system. 
Thermal  shell  option  (applies  only  to  thermal  and  coupled
structural  thermal  analyses).    See  parameter  THERM  on  DATA-
BASE_EXTENT_BINARY keyword. 
EQ.0: No temperature gradient is considered through the shell
thickness (default).   
EQ.1: A  temperature  gradient  is  calculated  through  the  shell 
thickness. 
|PSTUPD| is the optional shell part set ID specifying which part
ID’s  have  or  do  not  have  their  thickness  updated  according  to
ISTUPD.    The  shell  thickness  update  as  specified  by  ISTUPD  by
default applies to all shell elements in the mesh.   
LT.0:  these  shell  parts  are  excluded  from  the  shell  thickness
update   
EQ.0: all deformable shells have their thickness updated   
GT.0:  these  shell  parts  are  included  in  the  shell  thickness
update 
Shell part set ID for parts which use the type 4 thickness update
where  elastic  strains  are  ignored.    The  shell  parts  in  part  set
SIDT4TU  must  also  be  included  in  the  part  set  defined  by
PSTUPD.  SIDT4TU has no effect unless ISTUPD is set to 1 or 3. 
Flag affecting location of  contact surfaces for shells when NLOC
is  nonzero  in  *SECTION_SHELL  or  in  *PART_COMPOSITE,  or 
when  OFFSET  is  specified  using  *ELEMENT_SHELL_OFFSET. 
CNTCO is not supported for the slave side of NODES_TO_SUR-
FACE type contacts, neither has it any effect for Mortar contacts.
For Mortar contacts NLOC of OFFSET completely determines the
location of the contact surfaces, as if CNTCO = 1 would be set. 
EQ.0: NLOC  and  OFFSET  have  no  effect  on  location  of  shell
contact surfaces. 
EQ.1: Contact reference plane  coincides
with shell reference surface. 
EQ.2: Contact reference plane  is affected
VARIABLE   
DESCRIPTION
by contact thickness.  This is typically not physical. 
For automatic contact types, the shell contact surfaces are always,
regardless  of  CNTCO,  offset  from  a  contact  reference  plane  by
half  a  contact  thickness.    Contact  thickness  is  taken  as  the  shell
thickness  by  default  but  can  be  overridden,  for  example,  with 
input on Card 3 of *CONTACT. 
The  parameter  CNTCO  affects  how  the  location  of  the  contact
reference  plane  is  determined.    When  CNTCO = 0,  the  contact 
reference  plane  coincides  with  the  plane  of  the  shell  nodes.
Whereas when CNTCO = 1, the contact reference plane coincides 
with  the  shell  reference  surface  as  determined  by  NLOC  or  by
OFFSET.    For  CNTCO = 2,  the  contact  reference  plane  is  offset 
from the plane of the nodes by 
or by 
–
NLOC
× contact thickness 
OFFSET × (
contact thickness
shell thickness
) 
whichever applies. 
ITSFLG 
Flag  to  activate/deactivate  initial  transverse  shear  stresses  (local
shell  stress  components  𝜎𝑦𝑧  and  𝜎𝑧𝑥)  from  *INITIAL_STRESS_-
SHELL: 
EQ.0: keep transverse shear stresses 
EQ.1: set transverse shear stresses to zero 
IRQUAD 
In  plane  integration  rule  for  the  8-node  quadratic  shell  element 
(shell formulation 23): 
EQ.2: 2 × 2 Gauss quadrature (default), 
EQ.3: 3 × 3 Gauss quadrature.
Figure  12-86.    Illustration  of  an  element  in  a  W-Mode.    One  pair  of  opposite
corners  go  up,  and  the  other  pair  goes  down.    The  angle,  𝛼,  is  formed  by  the
plane of the flat element and by the vector connecting the center to the corner.
See Remark 4. 
  VARIABLE   
W-MODE 
STRETCH 
DESCRIPTION
W-Mode  amplitude  for  element  deletion,  specified  in  degrees.
See Figure 12-86 and Remark 4 for the definition of the angle. 
Stretch  ratio  of  element  diagonals  for  element  deletion.    This 
option  is  activated  if  and  only  if  either  NFAIL1  or  NFAIL4  are
nonzero and STRETCH > 0.0.  
ICRQ 
Continuous  treatment  across  element  edges  for  some  specified
result quantities.  See Remark 7.  
NFAIL1 
EQ.0: not active 
EQ.1: thickness and plastic strain 
Flag to check for highly distorted under-integrated shell elements, 
print a message, and delete the element or terminate.  Generally,
this flag is not needed for one point elements that do not use the
warping  stiffness.    A  distorted  element  is  one  where  a  negative 
Jacobian  exist  within  the  domain  of  the  shell,  not  just  at
integration  points.    The  checks  are  made  away  from  the  CPU
requirements for one point elements.  If nonzero, NFAIL1 can be
changed in a restart. 
EQ.1: print message and delete element.   
EQ.2: print message, write d3dump file, and terminate 
GT.2:  print  message  and  delete  element.    When  NFAIL1
elements  are  deleted  then  write  d3dump  file  and  termi-
nate.  These NFAIL1 failed elements also include all shell
elements  that  failed  for  other  reasons  than  distortion.
VARIABLE   
DESCRIPTION
NFAIL4 
PSNFAIL 
KEEPCS 
Before the d3dump file is written, NFAIL1 is doubled, so 
the run can immediately be continued if desired. 
Flag to check for highly distorted fully-integrated shell elements, 
print  a  message  and  delete  the  element  or  terminate.    Generally, 
this  flag  is  recommended.    A  distorted  element  is  one  where  a
negative Jacobian exist within the domain of the shell, not just at
integration  points. 
  The  checks  are  made  away  from  the
integration points to enable the bad elements to be deleted before 
an instability leading to an error termination occurs.  If nonzero, 
NFAIL4 can be changed in a restart. 
EQ.1: print message and delete element. 
EQ.2: print message, write d3dump file, and terminate 
GT.2:  print  message  and  delete  element.    When  NFAIL4 
elements  are  deleted  then  write  d3dump  file  and  termi-
nate.  These NFAIL4 failed elements also include all shell
elements  that  failed  for  other  reasons  than  distortion.
Before the d3dump file is written, NFAIL4 is doubled, so 
the run can immediately be continued if desired. 
Optional shell part set ID specifying which part ID’s are checked
by the NFAIL1, NFAIL4, and W-MODE options.  If zero, all shell 
part ID’s are included. 
Flag  to  keep  the  contact  segments  of  failed  shell  elements  in  the
calculation.    The  contact  segments  of  the  failed  shells  remain
active  until  a  node  shared  by  the  segments  has  no  active  shells
attached.  Only then are the segments deleted. 
EQ.0: Inactive 
EQ.1: Active 
DELFR 
Flag  to  delete  shell  elements  whose  neighboring  shell  elements
have failed; consequently, the shell is detached from the structure
and moving freely in space.  This condition is checked if NFAIL1
or NFAIL4 are nonzero. 
EQ.0: Inactive 
EQ.1: Isolated elements are deleted. 
EQ.2: Isolated  quadrilateral  elements  and  triangular  elements
connected by only one node are deleted.
VARIABLE   
DESCRIPTION
EQ.3: Elements  that  are  either  isolated  or  connected  by  only
one node are deleted. 
DRCPSID 
Part  set  ID  for  drilling  rotation  constraint  method  . 
DRCPRM 
Drilling rotation constraint parameter (default = 1.0). 
INTPERR 
Flag for behavior in case of unwanted interpolation/extrapolation
of initial stresses from *INITIAL_STRESS_SHELL. 
EQ.0: Only warning is written, calculation continues (default).
EQ.1: Error exit, calculation stops. 
Remarks: 
1.  Drill  versus  Full  Projections  for  Warping  Stiffness.    The  drill  projection  is 
used  in  the  addition  of  warping  stiffness  to  the  Belytschko-Tsay  and  the  Be-
lytschko-Wong-Chiang  shell  elements.    This  projection  generally  works  well 
and is very efficient, but to quote Belytschko and Leviathan: 
"The shortcoming of the drill projection is that even elements that are in-
variant  to  rigid  body rotation  will  strain  under  rigid  body  rotation  if  the 
drill projection is applied.  On one hand, the excessive flexibility rendered 
by the 1-point quadrature shell element is corrected by the drill projection, 
but on the other hand the element becomes too stiff due to loss of the rigid 
body rotation invariance under the same drill projection". 
They later went on to add in the conclusions: 
"The  projection  of  only  the  drill  rotations  is  very  efficient  and  hardly  in-
creases the computation time, so it is recommended for most cases.  How-
ever,  it  should  be  noted  that  the  drill  projection  can  result  in  a  loss  of 
invariance to rigid body motion when the elements are highly warped.  For 
moderately warped configurations the drill projection appears quite accu-
rate". 
In crashworthiness and impact analysis, elements that have little or no warpage 
in the reference configuration can become highly warped in the deformed con-
figuration and may affect rigid body rotations if the drill projection is used, i.e., 
DO  NOT  USE  THE  DRILL  PROJECTION.    Of  course  it  is  difficult  to  define 
what is meant by "moderately warped".  The full projection circumvents these 
problems but at a significant cost.  The cost increase of the drill projection ver-
sus no projection as reported by Belytschko and Leviathan is 12 percent and by
timings  in  LS-DYNA,  7  percent,  but  for  the  full  projection  they  report  a  110 
percent increase and in LS-DYNA an increase closer to 50 percent is observed. 
In Version 940 of LS-DYNA the drill projection was used exclusively, but in one 
problem the lack of invariance was observed; consequently, the drill projection 
was replaced in the Belytschko-Leviathan shell with the full projection and the 
full projection is now optional for the warping stiffness in the Belytschko-Tsay 
and  Belytschko-Wong-Chiang  elements.    Starting  with  version  950  the  Be-
lytschko-Leviathan shell, which now uses the full projection, is somewhat slow-
er  than  in  previous  versions.    In  general,  in  light  of  these  problems,  the  drill 
projection cannot be recommended.  For implicit calculations, the full projection 
method is used in the development of the stiffness matrix. 
2.  THEORY, ELFORM, and Contact with Tapered Shells.  All shell parts need 
not  share  the  same  element  formulation.    A  nonzero  value of  ELFORM,  given 
either  in  *SECTION_SHELL  or  *PART_COMPOSITE,  overrides  the  element 
formulation specified by THEORY in *CONTROL_SHELL.  
When  using  MPP,  THEORY = 1  in  *CONTROL_SHELL  has  special  meaning 
when  dealing  with  non-uniform-thickness  shells,  that  is,  it  serves  to  set  the 
nodal contact thickness equal to the average of the nodal thicknesses from the 
shells  sharing  that  node.    Thus  when  a  contact  surface  is  comprised  of  non-
uniform-thickness  shells,  THEORY = 1  is  recommended  and  the  user  still  has 
the  option  of  setting  the  actual  shell  theory  using  ELFORM  in  *SECTION_
SHELL. 
3.  Drilling Rotation Constraint Method.  The drilling rotation constraint method 
which  is  used  by  default  in  implicit  calculations   can be used in explicit calculations as well by 
defining an appropriate part set DRCPSID.  This might be helpful in situations 
where  single  constraints  (e.g.    spotwelds)  are  connected  to  flat  shell  element 
topologies.    The  additional  drill  force  can  by  scaled  with  DRCPRM  (default 
value is 1.0), where a moderate value should be chosen to avoid excessive stiff-
ening of the structure. A speed penalty of max.  15 % may be observed with this 
option. 
4.  W-Mode  Failure  Criterion.    The  w-mode  failure  criteria  depends  on  the 
magnitude of the w-mode, 𝑤, compared to the approximate side-length ℓ.  The 
magnitude, 𝑤, is defined as 
𝑤 =
[(𝐱1 − 𝐱2) + (𝐱3 − 𝐱4)] ⋅ 𝐧 
where  𝐱𝑖 is the position vector for node 𝑖, and 𝐧 is the element  normal vector 
evaluated at the centroid.  The element normal is the unit vector obtained from 
the cross product of the diagonal vectors 𝐚 and 𝐛 as,
𝐚 = 𝐱3 − 𝐱1 
𝐛 = 𝐱4 − 𝐱2 
𝐧 =
𝐚 × 𝐛
‖𝐚 × 𝐛‖
. 
The failure criteria depends on the ratio of 𝑤 to ℓ, where ℓ is defined as, 
ℓ =
⎤
⎡
⎥
⎢
√2 √
⎥
⎢
⎥
⎢
⎣
⎦
⏟⏟⏟⏟⏟⏟⏟
~diagonal length
‖𝐚 × 𝐛‖
⏟⏟⏟⏟⏟
~√area
such that the element is deleted when 
|𝑤|
≥ tan(WMODE). 
The angle 𝛼 in the figure may be identified as, 
α = arctan (
|𝑤|
). 
5.  2D Axisymmetric Solid Elements.  The 2D axisymmetric solid elements come 
in two types: area weighted (type 14) and volume weighted (type 15). 
a)  High  explosive  applications  work  best  with  the  area  weighted  approach 
and  structural  applications  work  best  with  the  volume  weighted  ap-
proach.    The  volume  weighted  approach  can  lead  to  problems  along  the 
axis  of  symmetry  under  very  large  deformations.    Often  the  symmetry 
condition is not obeyed, and the elements will kink along the axis. 
b)  The  volume  weighted  approach  must  be  used  if  2D  shell  elements  are 
used in the mesh.  Type 14 and 15 elements cannot be mixed in the same 
calculation. 
6.  Lamination  Theory.    Lamination  theory  should  be  activated  when  the 
assumption that shear strain through the shell is uniform and constant becomes 
violated.  Unless this correction is applied, the stiffness of the shell can be gross-
ly  incorrect  if  there  are  drastic  differences  in  the  elastic  constants  from  ply  to 
ply, especially for sandwich type shells.  Generally, without this correction the 
results  are  too  stiff.    For  the  discrete  Kirchhoff  shell  elements,  which  do  not 
consider  transverse  shear,  this  option  is  ignored.    For  thin  shells  of  material 
*MAT_ENHANCED_COMPOSITE_
types, 
DAMAGE,  and  *MAT_GENERAL_VISCOELASTIC,  laminated  shell  theory 
may also be done by stiffness correction by setting LAMSHT=1. 
*MAT_COMPOSITE_DAMAGE,
7.  Continuous  Result  Quantities.    A  nodal  averaging  technique  is  used  to 
achieve  continuity  for  some  quantities  across  element  edges.    Applying  this 
approach to the thickness field and plastic strains (ICRQ=1) can reduce alternat-
ing weak localizations sometimes observed in metal forming applications when 
shell elements get stretch-bended over small radii.  This option currently works 
with shell element types 2, 4, and 16.  A maximum number of 9 through thick-
ness integration points is allowed for this method.  A speed penalty of max.  15 
% may be observed with this option.
Purpose:  Provide controls for solid element response. 
*CONTROL 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ESORT 
FMATRX  NIPTETS  SWLOCL 
PSFAIL 
T10JTOL 
ICOH 
TET13K 
Type 
Default 
I 
0 
I 
0 
I 
4 
I 
1 
I 
0 
F 
0. 
I 
0 
I 
0 
This card is optional.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
PM1 
PM2 
PM3 
PM4 
PM5 
PM6 
PM7 
PM8 
PM9 
PM10 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none  none  none  none  none  none  none  none  none  none 
  VARIABLE   
ESORT 
DESCRIPTION
Automatic  sorting  of  tetrahedral  and  pentahedral  elements  to
avoid use of degenerate formulations for these shapes.  See *SEC-
TION_SOLID. 
EQ.0: no sorting (default) 
EQ.1: sort  tetrahedron  to  type  10;  pentahedron  to  type  15;
cohesive  pentahedron  types  19  and  20    to  types  21  and 
22, respectively. 
EQ.2: sort 
to 
tetrahedron 
integrated 
pentahedron to type 115; fully integrated pentahedron to
type 15; cohesive pentahedron types 19 and 20  to types
21 and 22, respectively. 
type  10;  1-point 
EQ.3: same as EQ.1 but also print switched elements in messag
file 
EQ.4: same as EQ.2 but also print switched elements in messag
file
FMATRX 
NIPTETS 
SWLOCL 
PSFAIL 
T10JTOL 
*CONTROL_SOLID 
DESCRIPTION
Default  method  used  in  the  calculation  of  the  deformation
gradient matrix. 
EQ.1: Update  incrementally  in  time.    This  is  the  default  for
explicit. 
EQ.2:  Directly compute F: 
This  is  the  default  for  implicit 
and implicit/explicit switching. 
Number  of  integration  points  used  in  the  quadratic  tetrahedron
elements.    Either  4  or  5  can  be  specified.    This  option  applies  to
the types 4, 16, and 17 tetrahedron elements. 
Output  option  for  stresses  in  solid  elements  used  as  spot  welds
with  material 
and 
d3plot/d3part/etc. 
*MAT_SPOTWELD. 
  Affects 
elout 
EQ.1: Stresses in global coordinate system (default), 
EQ.2: Stresses in element coordinate system. 
A  nonzero  PSFAIL  has  the  same  effect  as  setting  ERODE = 1  in 
*CONTROL_TIMESTEP except that solid element erosion due to 
negative  volume  is  limited  to  only  the  solid  elements  in  part  set 
PSFAIL. 
In  other  words,  when  PSFAIL  is  nonzero,  the  time-step-based 
criterion for erosion (TSMIN) applies to all solid elements (except
formulations  11  and  12)  while  the  negative  volume  criterion  for 
erosion applies only to solids in part set PSFAIL.  
Tolerance  for  jacobian  in  4-point  10-noded  quadratic  tetrahedra 
(type  16).    If  the  quotient  between  the  minimum  and  maximum
jacobian  value  falls  below  this  tolerance,  a  warning  message  is 
issued in the messag file.  This is useful for tracking badly shaped 
elements  in  implicit  analysis  that  deteriorates  convergence,  a
value of 1.0 indicates a perfectly shaped element.
VARIABLE   
ICOH 
TET13K 
PM1 – PM10 
DESCRIPTION
Global flag for cohesive element options, interpreted digit-wise as 
follows:  
ICOH = [𝐿𝐾] = 𝐾 + 10 × 𝐿 
K.EQ.1:  Solid elements having ELFORM = 19-22 will be eroded 
when  neighboring  shell  or  solid  elements  fail.    Only
works for nodewise connected parts, not tied contacts.
K.EQ.0:  No cohesive element deletion due to neighbor failure. 
L.EQ.0:   Default critical time step estimate. 
L.EQ.1:   Most  conservative 
estimate. 
(smallest)  critical 
time  step
L.EQ.2:  Intermediate critical time step estimate. 
Set  to  1  to  invoke  a  consistent  tangent  stiffness  matrix  for  the
pressure averaged tetrahedron (type 13).  This feature is available
only  for  the  implicit  integrator  and  it  is  not  supported  in  the 
MPP/MPI  version.    This  element  type  averages  the  volumetric
strain  over  adjacent  elements  to  alleviate  volumetric  locking,
therefore,  the  corresponding  material  tangent  stiffness  should  be
treated  accordingly.    In  contrast  to  a  hexahedral  mesh  where  a
node  usually  connects  to  fewer  than  8  elements,  tetrahedral
meshes  offer  no  such  regularity.    Consequently,  for  nonlinear
implicit  analysis  matrix  assembly  is  computationally  expensive
and  this  option  is  recommended  only  for  linear  or  eigenvalue
analysis  to  exploit  the  stiffness  characteristics  of  the  type  13
tetrahedron. 
Components of a permutation vector for nodes that define the 10-
node  tetrahedron.   The  nodal  numbering  of 10-node  tetrahedron 
elements  is  somewhat  arbitrary.    The  permutation  vector  allows
other  numbering  schemes  to  be  used.    Unless  defined,  this 
permutation vector is not used.  PM1 – PM10 are unique numbers 
between 1 to 10 inclusive that reorders the input node ID’s  for a
10-node tetrahedron into the order used by LS-DYNA.
*CONTROL_SOLUTION 
Purpose:  To specify the analysis solution procedure if thermal only or coupled thermal 
analysis is performed.  Other solutions parameters including the vector length and NaN 
(not a number) checking can be set. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SOLN 
NLQ 
ISNAN 
LCINT 
LCACC 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
100 
I 
0 
  VARIABLE   
DESCRIPTION
SOLN 
Analysis solution procedure: 
NLQ 
ISNAN 
LCINT 
EQ.0: Structural analysis only, 
EQ.1: Thermal analysis only, 
EQ.2: Coupled structural thermal analysis. 
Define  the  vector  length  used  in  solution.    This  value  must  not
exceed the vector length of the system which varies based on the
machine  manufacturer.    The  default  vector  length  is  printed  at
termination in the messag file. 
Flag to check for a NaN in the force and moment arrays after the
assembly of these arrays is completed.  This option can be useful
for debugging purposes.  A cost overhead of approximately 2% is
incurred when this option is active. 
EQ.0: No checking, 
EQ.1: Checking is active. 
Number  of  equally  spaced  points  used  in  curve  (*DEFINE_-
CURVE)  rediscretization.    Curve  rediscretization  applies  only  to
curves  used  in  material  models.    Curves  defining  loads,  motion,
etc.  are not rediscretized.
VARIABLE   
LCACC 
DESCRIPTION
Flag to truncate curves to 6 significant figures for single precision 
and 13 significant figures for double precision.  The truncation is
done  after  applying the  offset  and  scale  factors  specified  in  *DE-
FINE_CURVE.    Truncation  is  intended  to  prevent  curve  values
from  deviating  from  the  input  value,  e.g.,  0.7  being  stored  as
0.69999999.    This  small  deviation  was  seen  to  have  an  adverse
effect in a particular analysis using *MAT_083.  In general, curve 
truncation  is  not  necessary  and  is  unlikely  to  have  any  effect  on
results. 
EQ.0: No truncation. 
NE.0: Truncate.
*CONTROL_SPH 
Purpose:  Provide controls relating to SPH (Smooth Particle Hydrodynamics). 
  Card 1 
1 
2 
Variable 
NCBS 
BOXID 
Type 
Default 
I 
1 
I 
0 
3 
DT 
F 
4 
5 
6 
7 
8 
IDIM 
MEMORY
FORM 
START 
MAXV 
I 
I 
1020 
none 
150 
I 
0 
F 
F 
0.0 
1015 
Optional Card. 
  Card 2 
1 
2 
Variable 
CONT 
DERIV 
Type 
Default 
I 
0 
I 
0 
3 
INI 
I 
0 
4 
5 
6 
7 
8 
ISHOW 
IEROD 
ICONT 
IAVIS 
ISYMP 
I 
0 
I 
0 
I 
0 
I 
0 
I 
100 
  VARIABLE   
DESCRIPTION
NCBS 
Number of time steps between particle sorting. 
BOXID 
DT 
IDIM 
SPH approximations are computed inside a specified BOX.  When
a  particle  has  gone  outside  the  BOX,  it  is  deactivated.    This  will
save  computational  time  by  eliminating  particles  that  no  longer
interact with the structure. 
Death time.  Determines when the SPH calculations are stopped. 
Space dimension for SPH particles: 
EQ.3:  for 3D problems 
EQ.2:  for 2D plane strain problems 
EQ.-2: for 2D axisymmetric problems 
MEMORY 
Defines the initial number of neighbors per particle .
VARIABLE   
DESCRIPTION
FORM 
Particle approximation theory (Remark 2): 
EQ.0: default formulation 
EQ.1: renormalization approximation 
EQ.2: symmetric formulation 
EQ.3: symmetric renormalized approximation 
EQ.4: tensor formulation 
EQ.5: fluid particle approximation 
EQ.6: fluid particle with renormalization approximation 
EQ.7: total Lagrangian formulation 
EQ.8: total Lagrangian formulation with renormalization  
EQ.15: enhanced fluid formulation 
EQ.16: enhanced fluid formulation with renormalization 
Start  time  for  particle  approximation.    Particle  approximations
will be computed when time of the analysis has reached the value
defined in START. 
Maximum value for velocity for the SPH particles.  Particles with 
a velocity greater than MAXV are deactivated.  A negative MAXV
will turn off the velocity checking. 
Defines  the  computation  of  the  particle  approximation  between
different SPH parts: 
EQ.0: Particle approximation is defined (default) 
EQ.1: Particle  approximation  is  not  computed.    Different  SPH
materials  will  not  interact  with  each  other  and  penetra-
tion  is  allowed  unless  *DEFINE_SPH_TO_SPH_COU-
PLING is defined.  Combined with *SECTION_SPH_IN-
TERACTION,  a  partial  interaction  between  SPH  parts 
through  normal  interpolation  method  and  partially  in-
teract  through  the  contact  option  can  be  realized.    See
*SECTION_SPH_INTERACTION. 
START 
MAXV 
CONT 
DERIV 
Time integration type for the smoothing length: 
EQ.0:  𝑑
EQ.1:  𝑑
𝑑𝑡 [ℎ(𝑡)] = 1
𝑑𝑡 [ℎ(𝑡)] = 1
𝑑 ℎ(𝑡)∇ ⋅ 𝐯, (default), 
𝑑 ℎ(𝑡)(∇ ⋅ 𝐯)1/3
VARIABLE   
DESCRIPTION
INI 
Computation of the smoothing length during the initialization: 
EQ.0: Bucket sort based algorithm (default, very fast). 
EQ.1: Global computation on all the particles of the model. 
EQ.2: Based on the mass of the SPH particle. 
ISHOW 
Display option for deactivated SPH particles: 
EQ.0: No  distinction  in  active  SPH  particles  and  deactivated
SPH particles when viewing in LS-PrePost. 
EQ.1: Deactivated  SPH  particles  are  displayed  only  as  points
and  active  SPH  particles  are  displayed  as  spheres  when 
Setting → SPH → Style is set to “smooth” in LS-PrePost. 
IEROD 
Deactivation control for SPH particles: 
EQ.0: Particles remain active. 
EQ.1: SPH  particles  are  partially  deactivated  and  stress  states
are  set  to  0  when  erosion  criteria  are  satisfied.    See  Re-
mark 3. 
EQ.2:  SPH particles are totally deactivated and stress states are
set to 0 when erosion criteria are satisfied.  See Remark 3.
ICONT 
Controls contact behavior for deactivated SPH particles: 
EQ.0: Any  contact  defined  for  SPH  remains  active  for
deactivated particles. 
EQ.1: Contact is inactive for deactivated particles. 
IAVIS 
Defines artificial viscosity formulation for SPH elements (Remark 
4): 
ISYMP 
EQ.0: Monaghan type artificial viscosity formulation is used. 
EQ.1: Standard  type  artificial  viscosity  formulation  from  solid
element is used (this option is not supported in SPH 2D
and 2D axisymmetric elements). 
Defines the percentage of original SPH particles used for memory 
allocation  of  SPH  symmetric  planes  ghost  nodes  generation
process (default is 100%).  Recommended for large SPH particles
models (value range 10~20) to control the memory allocation for
SPH  ghost  particles  with  *BOUNDARY_SPH_SYMMETRY_-
PLANE keyword.
*CONTROL 
1.  Memory.  MEMORY is used to determine the initial memory allocation for the 
SPH  arrays.    Its  value  can  be  positive  or  negative.    If  MEMORY  is  positive, 
memory allocation is dynamic such that the number of neighboring particles is 
initially equal to MEMORY but that number is subsequently allowed to exceed 
MEMORY as the solution progresses.  If MEMORY is negative, memory alloca-
tion is static and |MEMORY| is the maximum allowed number of neighboring 
particles  for  each  particle  throughout  the  entire  solution.    Using  this  static 
memory option can avoid memory allocation problems. 
2.  Form.    Some  guidelines  for  selecting  form  variable:      for  most  solid  structure 
applications,  form  =  1  is  recommended  for  more  accurate  results  around  the 
boundary area;   for fluid or fluid-like material applications, form = 15, 16 with 
fluid  formulation  are  recommended  (form=16  usually  has  better  accuracy  but 
requires more CPU time);   form = 2, 3 are not recommended for any case;   all 
SPH  formulations  with  Eulerian  kernel  (form  =  0  to  6,  15  and  16)  can  be  used 
for large or extreme large deformation applications but will have tensile insta-
bility issue;   all SPH formulations with Lagrangian kernel (form = 7,8) can be 
used to avoid tensile instability issue but they can not endure very large defor-
mation, user has to be careful to pick up the right one based on the applications.  
Only formulations 0, 1, 15 and 16 are implemented for 2D axisymmetric prob-
lems (dim=-2).  Also note that forms 15 and 16 include a smoothing of the pres-
sure  field,  and  are  therefore  not  recommended  for  materials  with  failure  or 
problems with important strain localization. 
3.  Erosion.    The  erosion  criteria,  which  triggers  particle  deactivation  when 
IEROD=1  or  2,  may  come  from  either  the  material  model  with  *MAT_ADD_-
EROSION or from the ERODE parameter in *CONTROL_TIMESTEP.  For IER-
OD=1,  SPH  particles  are  partially  deactivated    (i.e.    the  stress  states  of  the 
deactivated SPH particles will be set to 0, but those particles still remain in the 
domain  integration  for  more  stable  results);  For  IEROD=2,  SPH  particles  are 
totally deactivated: stress states will be set to 0 and the deactivated particles no 
more  remain  in  the  domain  integration.    Deactivated  particles  can  be  distin-
guished from active particles by setting ISHOW=1.  To disable contact for deac-
tivated particles, set ICONT=1. 
4.  Artificial Viscosity.  The artificial viscosity for standard solid elements, which 
is active when AVIS=1, is given by: 
2 − 𝑄2𝑎𝜀̇𝑘𝑘)
𝑞 = 𝜌𝑙(𝑄1𝑙𝜀̇𝑘𝑘
𝑞 = 0
𝜀̇𝑘𝑘 < 0
𝜀̇𝑘𝑘 ≥ 0
where  𝑄1  and  𝑄2  are  dimensionless  input  constants  which  default  to  1.5  and 
.06, respectively, and 𝑙 is a characteristic length given as the square root of the 
area in two dimensions and as the cube root of the volume in three, 𝑎 is the local
sound speed.  This formulation, which is consistent with solid artificial viscosi-
ty, has better energy balance for SPH elements.  For general applications, Mon-
aghan  type  artificial  viscosity  is  recommended  since  this  type  of  artificial 
viscosity is specifically designed for SPH particles. 
The  Monaghan  type  artificial  viscosity,  which  is  active  when  AVIS = 0,  is  de-
fined as follows: 
𝑞 =
⎧−𝑄2𝑐𝑖𝑗𝜙𝑖𝑗 + 𝑄1𝜙𝑖𝑗
{{
𝜌𝑖𝑗
⎨
{{
⎩
𝑣𝑖𝑗𝑥𝑖𝑗 < 0
𝑣𝑖𝑗𝑥𝑖𝑗 ≥ 0
Where, 
𝜙𝑖𝑗 =
ℎ𝑖𝑗𝑣𝑖𝑗𝑥𝑖𝑗
∣𝑥𝑖𝑗∣
+ 𝜑2
𝑐 ̅𝑖𝑗 = 0.5(𝑐𝑖 + 𝑐𝑗) 
𝜌̅𝑖𝑗 = 0.5(𝜌𝑖 + 𝜌𝑗) 
ℎ𝑖𝑗 = 0.5(ℎ𝑖 + ℎ𝑗) 
𝜑 = 0.1ℎ𝑖𝑗 
𝑄1, 𝑄2 are input constants.  When using Monaghan type artificial viscosity, it is 
recommended  that  the  user  set  both  Q1  and  Q2  to  1.0  on  either  the  *CON-
TROL_BULK_VISCOSITY  or  *HOURGLASS  keywords;  see  for  example  G.    R.  
Liu.
*CONTROL 
Purpose:  Provides factors for scaling the failure force resultants of beam spot welds as a 
function of their parametric location on the contact segment and the size of the segment.  
Also,  an  option  is  provided  to  replace  beam  welds  with  solid  hexahedron  element 
clusters. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCT 
LCS 
T_ORT 
PRTFLG 
T_ORS 
RPBHX 
BMSID 
ID_OFF 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
LCT 
LCS 
T_ORT 
PRTFLG 
Load  curve  ID  for  scaling  the  response  in  tension  based  on  the
shell element size. 
Load curve ID for scaling the response in shear based on the shell
element size. 
Table  ID  for  scaling  the  tension  response  (and  shear  response  if
T_ORS = 0) based on the location of the beam node relative to the
centroid of the shell. 
Set this flag to 1 to print for each spot weld attachment: the beam,
node,  and  shell  ID’s,  the  parametric  coordinates  that  define  the
constraint  location,  the  angle  used  in  the  table  lookup,  and  the
three  scale  factors  obtained  from  the  load  curves  and  table 
lookup.  See Figure 12-87.  
Figure 12-87.  Definition of parameters for table definition.
VARIABLE   
DESCRIPTION
Optional  table  ID  for  scaling  the  shear  response  based  on  the
location of the beam node relative to the centroid of the shell. 
Replace  each  spot  weld  beam  element  with  a  cluster  of  RPBHX 
solid elements.  The net cross-section of the cluster of elements is 
dimensioned to have the same area as the replaced beam.  RPBHX 
may  be  set  to  1,  4,  or 8.    When  RPBHX  is  set  to  4 or  8,  a  table  is 
generated  to  output  the  force  and  moment  resultants  into  the
SWFORC  file,  if  this  file  is  active.    This  table  is  described  by  the
keyword: *DEFINE_HEX_SPOTWELD_ASSEMBLY.   The ID’s of 
the  beam  elements  are  used  as  the  cluster  spot  weld  ID’s  so  the
ID’s in the SWFORC file are unchanged.  The beam elements are
automatically  deleted  from  the  calculation,  and  the  section  and
material  data  is  automatically  changed  to  be  used  with  solid
elements.  See Figure 11-24. 
Optional beam set ID defining the beam element ID’s that are to
be  converted  to  hex  assemblies.    If  zero,  all  spot  weld  beam 
elements are converted to hex assemblies. 
This  optional  ID  offset  applies  if  and  only  if  BMSID  is  nonzero. 
Beams,  which  share  part  ID’s  with  beams  that  are  converted  to
hex  assemblies,  will  be  assigned  new  part  ID’s  by  adding  to  the
original part ID the value of ID_OFF.  If ID_OFF, is zero the new 
part  ID  for  such  beams  will  be  assigned  to  be  larger  than  the
largest part ID in the model. 
T_ORS 
RPBHX 
BMSID 
ID_OFF 
Remarks: 
The  load  curves  and  table  provide  a  means  of  scaling  the  response  of  the  beam  spot 
welds  to  reduce  any  mesh  dependencies  for  failure  model  6  in  *MAT_SPOTWELD.   
Figure  12-88  shows  such  dependencies  that  can  lead  to  premature  spot  weld  failure.  
Separate scale factors are calculated for each of the beam’s nodes.  The scale factors sT, 
sS, sOT , and sOS are calculated using the load curves LCT, LCS, table T_ORT, and table 
T_ORS, respectively, and are introduced in the failure criteria,  
⎢⎡𝑠𝑇𝑠𝑂𝑇𝜎𝑟𝑟
⎥⎤
𝐹 (𝜀̇𝑒𝑓𝑓 )⎦
𝜎𝑟𝑟
⎣
+
⎢⎡ 𝑠𝑆𝑠𝑂𝑆𝜏
⎥⎤
𝜏𝐹(𝜀̇𝑒𝑓𝑓 )⎦
⎣
− 1 = 0 
If a curve or table is given an ID of 0, its scale factor is set to 1.0.  The load curves LCT 
and LCS are functions of the characteristic size of the shell element used in the time step 
calculation at the start of the calculation.  The orientation table is a function of the spot 
weld’s  isoparametric  coordinate  location  on  the  shell  element.    A  vector  V=(s,t)  is
defined  from  the  centroid  of  the  shell  to  the  contact  point  of  the  beam’s  node.    The 
arguments for the orientation table are the angle: 
Θ = tan−1 [
min(|𝑠|, |𝑡|)
max(|𝑠|, |𝑡|)
], 
and  the  normalized  distance  𝑑 ̅= 𝑑
𝐷⁄ = max(|𝑠|, |𝑡|).      See  Figure  12-87    The  table  is 
periodic over a range of 0 (V aligned with either the s or t axis) to 45 degrees (V is along 
the diagonal of the element).  The table is specified by the angle of V in degrees, ranging 
from  0  to  45,  and  the  individual  curves  give  the  scale  factor  as  a  function  of  the 
normalized distance of the beam node, 𝑑̅̅̅̅̅̅ , for a constant angle.
1.20
1.00
0.80
0.60
0.40
0.20
0.00
1.20
1.00
0.80
0.60
0.40
0.20
0.00
_
.
_
.
CROSS TENSION
EDGE DIRECTION
.
1.20
1.00
0.80
0.60
0.40
0.20
0.00
Both side
One side
dynamic
static
10
12
            Center     Point1     Point2      Point3     Point4      Edge
MESH SIZE (mm)
SHEAR
dynamic
static
SPOT BEAM LOCATION
CORNER DIRECTION
Both side
One side
.
1.20
1.00
0.80
0.60
0.40
0.20
0.00
10
12
MESH SIZE (mm)
             Center     Point1       Point2    Point3     Point4     Corner
SPOT BEAM LOCATION
Figure 12-88  The failure force resultants can depend both on mesh size and 
the location of weld relative to the center of the contact segment
Purpose:  Define the start time of analysis. 
*CONTROL 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BEGTIM 
Type 
F 
  VARIABLE   
BEGTIM 
DESCRIPTION
Start time of analysis (default = 0.0).  Load curves are not shifted to 
compensate for the time offset.  Therefore, this keyword will change 
the  results  of  any  calculation  involving  time-dependent  load 
curves.
*CONTROL_STAGED_CONSTRUCTION 
This  control  card  is  used  to  help  break  down  analyses  of  construction  processes  into 
stages. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TSTART 
STGS 
STGE 
ACCEL 
FACT 
STREF 
DORDEL  NOPDEL 
Type 
Default 
F 
0 
I 
0 
I 
0 
F 
F 
0.0 
1.e-6 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
TSTART 
Time at start of analysis (normally leave blank) 
STGS 
STGE 
Construction stage at start of analysis 
Construction stage at end of analysis 
ACCEL 
Default acceleration for gravity loading 
FACT 
Default  stiffness  and  gravity  factor  for  parts  before  they  are
added 
STREF 
Reference stage for displacements in d3plot file 
DORDEL 
Dormant part treatment in d3plot file, see notes. 
EQ.0: Parts not shown when dormant (flagged as “deleted”), 
EQ.1: Parts shown normally when dormant. 
NOPDEL 
Treatment of pressure loads on deleted elements, see notes. 
EQ.0: Pressure loads automatically deleted, 
EQ.1: No automatic deletion.
Remarks: 
See  also  *DEFINE_CONSTRUCTION_STAGES  and  *DEFINE_STAGED_CONSTRUC-
TION_PART. 
The  staged  construction  options  offer  flexibility  to  carry  out  the  whole  construction 
simulation  in  one  analysis,  or  to  run  it  stage  by  stage.    Provided  that  at  least  one 
construction stage is defined (*DEFINE_CONSTRUCTION_STAGES), a dynain file will 
be  written  at  the  end  of  each  stage  (file  names  are  end_stage001_dynain,  etc).    These 
contain node and element definitions and the stress state; the individual stages can then 
be re-run without re-running the whole analysis.  To do this, make a new input file as 
follows: 
•  Copy  the  original  input  file,  containing  *DEFINE_CONSTRUCTION_-
STAGES and *DEFINE_STAGED_CONSTRUCTION_PART. 
•  Delete node and element definitions as these will be present in the dynain file 
(*NODE, *ELEMENT_SOLID, *ELEMENT_SHELL, and *ELEMENT_BEAM). 
•  Delete  any  *INITIAL  cards;  the  initial  stresses  in  the  new  analysis  will  be 
taken from the dynain file. 
•  On *CONTROL_STAGED_CONSTRUCTION set STGS to start at the desired 
stage 
•  Add an *INCLUDE statement referencing, for example, end_stage002_dynain 
if starting the new analysis from Stage 3. 
•  Move or copy the dynain file into the same directory as the new input file. 
When STGS is > 1 the analysis starts at a non-zero time (the start of stage STGS).  In this 
case a dynain file must be included to start the analysis from the stress state at the end 
of the previous stage.  The end time for stage STGE overrides the termination time on 
*CONTROL_TERMINATION.  A new dynain file will be written at the end of all stages 
from STGS to STGE. 
ACCEL and FACT are used with *STAGED_CONSTRUCTION_PART for simpler input 
definition of the parts present at different construction stages. 
If STGS > 1 and elements have been deleted in a previous stage, these elements will be 
absent from the new analysis and should not be referred to (e.g.  *DATABASE_HISTO-
RY_SOLID) in the new input file. 
TSTART can be used to set a non-zero start time (again, assuming a compatible dynain 
file is included).  This option is used only if construction stages have not been defined.
STREF allows the user to set a construction stage at the start of which displacements are 
considered to be zero – e.g.  so that initial analysis stages that achieve a pre-construction 
equilibrium do not contribute to contour plots of displacement.  The current coordinates 
are  not  modified,  only  the  “initial  geometry”  coordinates  in  the  d3plot  file.    If  this 
analysis starts from a stage later than STREF, the reference geometry will be taken from 
the dynain file that was written at the end of the stage previous to STREF – this dynain 
file must be in the same directory as the current model for this process to occur.  This 
feature is not available in MPP. 
DORDEL:  By  default,  parts  for  which  *DEFINE_STAGED_CONSTRUCTION_PART  is 
defined are flagged as “deleted” in the d3plot file at time-states for which the part is not 
active (i.e.  STGA has not yet been reached).  Parts that are deleted because STGR has 
been  reached  are  also  flagged  as  “deleted”.    When  animating  the  results,  the  parts 
should appear as they become active and disappear as they are deleted.  If DORDEL is 
non-zero, inactive parts (before STGA) are shown normally.  The parts are still shown 
as deleted after STGR is reached. 
NOPDEL: By default, pressure load “segments” are automatically deleted by LS-DYNA 
if they share all four nodes with a deleted solid or shell element.  In staged construction, 
the  user  may  want  to  apply  pressure  load  to  the  surface  of  an  element  (A)  that  is 
initially  shared  with  an  element  (B),  where  B  is  deleted  during  the  calculation.    For 
example, B may be in a layer of soil that is excavated, leaving A as the new top surface.  
The default scheme would delete the pressure segment when B is removed, despite the 
fact that A is still present.  NOPDEL instructs LS-DYNA to skip the automatic deletion 
of  pressure  segments,  irrespective  of  whether  the  elements  have  been  deleted  due  to 
staged construction or material failure.  The user must then ensure that pressure loads 
are not applied to nodes no longer supported by an active element.
*CONTROL_STEADY_STATE_ROLLING 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IMASS 
LCDMU 
LCDMUR 
IVEL 
SCL_K 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
  VARIABLE   
DESCRIPTION
IMASS 
Inertia switching flag 
EQ.0: include inertia during an implicit dynamic simulation. 
EQ.1: treat  steady  state  rolling  subsystems  as  quasi-static 
during implicit dynamic simulations. 
LCDMU 
Optional load curve for scaling the friction forces in contact. 
LCDMUR 
Optional  load  curve  for  scaling  the  friction  forces  in  contact
during dynamic relaxation.  If  LCDMUR isn’t specified, LCDMU
is used. 
IVEL 
Velocity switching flag. 
EQ.0: eliminate the steady state rolling body forces and set the 
velocities of the nodes after dynamic relaxation. 
EQ.1: keep  the  steady  state  rolling  body  forces  after  dynamic
relaxation instead of setting the velocities. 
Scale  factor  for  the  friction  stiffness  during  contact  loading  and 
unloading.    The  default  values  are  1.0  and  0.01  for  explicit  and
implicit,  respectively.    Any  scaling  applied  here  applies  only  to
contact involving the subsystem of parts defined for steady state
rolling. 
SCL_K 
Remarks: 
1.  Treating  the  steady  state  rolling  subsystems  as  quasi-static  during  an  implicit 
simulation may eliminate vibrations in the system that are not of interest and is 
generally recommended.
2.  Ramping  up  the  friction  by  scaling  it  with  LCDMU  and  LCDMUR  may 
improve  the  convergence  behavior  of  implicit  calculations.    The  values  of  the 
load curves should be 0.0 at initial contact and ramp up smoothly to a value of 
1.0.  
3.  After dynamic relaxation, the default behavior is to initialize the nodes with the 
velocities  required  to  generate  the  body  forces  on  elements  and  remove  the 
body  forces.    This  initialization  is  skipped,  and  the  body  forces  retained,  after 
dynamic relaxation if IVEL = 1. 
4.  The  friction  model  in  contact  is  similar  to  plasticity,  where  there  is  an  elastic 
region  during  the  loading  and  unloading  of  the  friction  during  contact.    The 
elastic stiffness is scaled from the normal contact stiffness.  For implicit calcula-
tions, the default scale factor is 0.01, which results in long periods of time being 
required to build the friction force, and, in some cases, oscillations in the contact 
forces.  A value between 10 and 100 produces smoother solutions and a faster 
build-up and decay of the friction force as the tire velocity or slip angle is var-
ied, allowing a parameter study to be performed in a single run.
*CONTROL_STRUCTURED_{OPTION} 
Available options include: 
<BLANK> 
TERM 
Purpose:    Write  out  an  LS-DYNA  structured  input  deck  that  is  largely  or  wholly 
equivalent to the keyword input deck.  This option may be useful in debugging errors 
that occur during processing of the input file, particularly if error messages of the type 
“*** ERROR ##### (STR + ###)” are written.  The name of the structured input deck is 
“dyna.str”. 
Not all LS-DYNA features are supported in structured input format.    Some data such 
as load curve numbers will be output in an internal numbering system.   
If the TERM option is activated, termination will occur after the structured input deck is 
written.   
Adding  “outdeck = s”  to  the  LS-DYNA  execution  line  serves  the  same  purpose  as 
including *CONTROL_STRUCTURED in the keyword input deck.
*CONTROL_SUBCYCLE_{K}_{L} or 
*CONTROL_SUBCYCLE_{OPTION} 
Available options for subcycling first form with K and L 
𝐾, 𝐿 ∈ {<BLANK>, 1, 2, 4, 8, 16, 32, 64}  
Available options for multiscale (OPTION) include: 
<BLANK> 
MASS_SCALED_PART 
MASS_SCALED_PART_SET 
Purpose:  This keyword is used to activate subcycling or mass scaling (multiscale).  The 
common  characteristic  of  both  methods  is  that  the  time  step  varies  from  element  to 
element, thereby eliminating unnecessary stepping on more slowly evolving portions of 
the model.  These techniques are suited for reducing the computational cost for models 
involving large spatial variation in mesh density and/or material characteristics. 
Subcycling is described in the LS-DYNA Theory Manual and in detail in Borrvall et.al.  
[2014]  and  may  be  seen  as  an  alternative  to  using  selective  mass  scaling,  see  the 
keyword *CONTROL_TIMESTEP. 
This keyword comes in two variations: 
1.  Subcycling.  Plain subcycling is activated by the *CONTROL_SUBCYCLE_{𝐾}_
{𝐿} variant of this keyword.  This form of the card should not be included more 
than  once.    It  may  be  used  in  conjunction  with  mass  scaling  to  limit  the  time 
step characteristics. 
For  subcycling,  time  steps  for  integration  are  determined  automatically  from 
the  characteristic  properties  of  the  elements  in  the  model,  with  the  restriction 
that the ratio between the largest and smallest time step is limited by  𝐾.  Fur-
thermore, 𝐿  determines  the  relative  time  step  at  which  external  forces  such  as 
contacts and loads are calculated 
For  example,  *CONTROL_SUBCYCLE_16_4  limits  the  largest  explicit  integra-
tion  time  step  to  at  most  16  times  the  smallest.    Contact  forces  are  evaluated 
every  4 time  steps.    The  defaults  are 𝐾 = 16  and 𝐿 = 1,  and  L  cannot  be  speci-
fied larger than 𝐾.  This option may be used without mass scaling activated but 
internally elements may still be slightly mass scaled to maintain computational 
efficiency. 
2.  Mass  Scaling/Multiscale.    For  a  multiscale  simulation,  mass  scaling  is 
mandatory and the time steps are directly specified in the input.  The specified
parts    or  part  sets    run  at  the  time  step 
specified  in  the  TS  field.    All  other  elements  evolve  with  a  time  step  set  by 
|DT2MS|, which is set on *CONTROL_TIMESTEP card. 
This feature was motivated by automotive crash simulation, wherein it is com-
mon  for  a  small  subset  of  solid  elements  to  limit  the  time  step  size.    With  this 
card the finely meshed parts (consisting of solid elements) can be made to run 
with a smaller time step through mass scaling so that the rest of the vehicle can 
run with a time step size of |DT2MS|. 
Part  Card.    Additional  card  for  the  MASS_SCALED_PART  and  MASS_SCALED_-
PART_SET  keyword  options.    Provide  as  many  cards  as  necessary.    Input  ends  at  the
next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID/PSID 
TS 
Type 
I 
F 
Default 
none 
none 
  VARIABLE   
DESCRIPTION
PID/PSID 
Part ID or part set ID if the SET option is specified. 
TS 
Time  step  size  at  which  mass  scaling  is  invoked  for  the  PID  or 
PSID
Purpose:  Stop the job. 
*CONTROL_TERMINATION 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ENDTIM 
ENDCYC 
DTMIN 
ENDENG  ENDMAS  NOSOL 
Type 
F 
Default 
0.0 
I 
0 
F 
F 
F 
0.0 
0.0 
1.0E+08
I 
0 
Remarks 
1 
2 
  VARIABLE   
DESCRIPTION
ENDTIM 
Termination time.  Mandatory. 
ENDCYC 
DTMIN 
ENDENG 
ENDMAS 
Termination cycle.  The termination cycle is optional and will be
used if the specified cycle is reached before the termination time.
Cycle number is identical with the time step number. 
Reduction  (or  scale)  factor  to  determine  minimum  time  step,
tsmin,  where   tsmin= dtstart× DTMIN  and  dtstart    is  the  initial 
step size determined  by LS-DYNA.  When the time step drops to 
tsmin,  LS-DYNA  terminates  with  a  restart  dump.    See  the
exception  described in Remark 2. 
Percent  change  in  energy  ratio  for  termination  of  calculation.    If 
undefined, this option is inactive. 
Percent  change  in  the  total  mass  for  termination  of  calculation.
This option is relevant if and only if mass scaling is used to limit
the minimum time step size, see *CONTROL_TIMESTEP variable 
name “DT2MS”. 
NOSOL 
Flag for a non-solution run, i.e.  normal termination directly after
initialization. 
EQ.0: off (default), 
EQ.1: on.
Remarks: 
1.  Termination by displacement may be defined in the *TERMINATION section. 
2. 
If  the  erosion  flag  on  *CONTROL_TIMESTEP  is  set  (ERODE = 1),  then  solid 
elements  and  thick  shell  elements  whose  time  step  falls  below  tsmin  will  be 
eroded  and  the  analysis  will  continue.    This  time-step-based  failure  option  is 
not recommended when solid formulations 11 or 12 are included in the model.  
Furthermore, when PSFAIL in *CONTROL_SOLID is nonzero, regardless of the 
value of ERODE, then all solid elements excepting those with formulation 11 or 
12, whose time step falls below tsmin will be eroded and the analysis will con-
tinue.    This  time-step-based  erosion  of  solids  due  to  a  nonzero  PSFAIL  is  not 
limited to solids in part set PSFAIL.   Only the negative-volume-based erosion 
criterion is limited to solids in part PSFAIL.
*CONTROL_THERMAL_EIGENVALUE 
Purpose:    Compute  eigenvalues  of  thermal  conductance  matrix  for  model  evaluation 
purposes. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NEIG 
Type 
Default 
I 
0 
. 
. 
  VARIABLE   
DESCRIPTION
NEIG 
Number of eigenvalues to compute. 
EQ.0: No eigenvalues are computed. 
GT.0: Compute NEIG eigenvalues of each thermal conductance
matrix. 
Remarks: 
1.  Computes  NEIG  eigenvalues  for  each  thermal  conductance  matrix.    This  is  a 
model evaluation tool and it is recommended that only a small number, such as 
1, thermal time steps are used when using this feature.
*CONTROL_THERMAL_NONLINEAR 
Purpose:    Set  parameters  for  a  nonlinear  thermal  or  coupled  structural/thermal 
analysis.  The control card, *CONTROL_SOLUTION, is also required. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
REFMAX 
TOL 
DCP 
LUMPBC 
THLSTL 
NLTHPR 
PHCHPN 
Type 
I 
F 
F 
Default 
10 
1.e-04  1.0 or 0.5
I 
0 
F 
0. 
I 
0 
F 
100. 
  VARIABLE   
DESCRIPTION
REFMAX 
Maximum number of matrix reformations per time step: 
EQ.0: set to 10 reformations. 
TOL 
Convergence tolerance for temperature: 
EQ.0.0: set to 1000 * machine roundoff. 
DCP 
Divergence control parameter: 
steady state problems   0.3 ≤ DCP ≤ 1.0 
0.0 < DCP ≤ 1.0 
transient problems  
default 1.0 
default 0.5 
LUMPBC 
Lump  enclosure  radiation  boundary  condition.    LUMPBC = 1 
activates  a  numerical  method 
to  damp  out  anomalous
temperature  oscillations  resulting  from  very  large  step  function
boundary conditions.  This option is not generally recommended.
EQ.0: off (default) 
EQ.1: on 
THLSTL 
Line search convergence tolerance: 
EQ.0.0: No line search 
GT.0.0: Line search convergence tolerance
VARIABLE   
DESCRIPTION
NLTHPR 
Thermal nonlinear print out level: 
EQ.0: No print out 
EQ.1: Print  convergence  parameters  during  solution  of
nonlinear system 
PHCHPN 
Phase change penalty parameter: 
EQ.0.0: Set to default value 100. 
GT.0.0: Penalty to enforce constant phase change temperature
*CONTROL 
Purpose:  Set options for the thermal solution in a thermal only or coupled structural-
thermal analysis.  The control card, *CONTROL_SOLUTION, is also required. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ATYPE 
PTYPE 
SOLVER 
CGTOL 
GPT 
EQHEAT 
FWORK 
SBC 
Type 
Default 
I 
0 
I 
0 
I 
F 
3 
10-4/10-6
I 
8 
F 
1. 
F 
1. 
Remaining cards are optional.† 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
Variable  MSGLVL  MAXITR 
ABSTOL 
RELTOL 
OMEGA 
Type 
Default 
I 
0 
I 
F 
F 
F 
500 
10-10 
10-6 
1.0 or 0.
F 
0. 
8 
TSF 
F 
1. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MXDMP 
DTVF 
VARDEN 
Type 
Default 
I 
0 
F 
0. 
I 
0 
.
*CONTROL_THERMAL_SOLVER 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MSGLVL  NINNER 
ABSTOL 
RELTOL  NOUTER 
Type 
Default 
I 
0 
I 
F 
F 
I 
100 
10-10 
10-6 
100 
  VARIABLE   
DESCRIPTION
ATYPE 
Thermal analysis type: 
EQ.0:  Steady state analysis, 
EQ.1:  transient analysis. 
PTYPE 
Thermal  problem  type:   
EQ.0:  linear problem, 
EQ.1:  nonlinear problem with material properties evaluated at 
gauss point temperature. 
EQ.2:  nonlinear problem with material properties evaluated at
element average temperature.
VARIABLE   
DESCRIPTION
SOLVER 
Thermal analysis solver type: 
EQ.1:  using solver 11 (enter -1 to use the old ACTCOL solver),
EQ.2:  nonsymmetric direct solver, 
EQ.3:  diagonal scaled conjugate gradient iterative (default), 
EQ.4: 
incomplete choleski conjugate gradient iterative, 
EQ.5:  nonsymmetric diagonal scaled bi-conjugate gradient 
EQ.11:  symmetric direct solver 
For MPP executables: 
EQ.11:  symmetric direct solver, 
EQ.12:  diagonal  scaling  (default  for  mpp)  conjugate  gradient
iterative, 
EQ.13:  symmetric Gauss-Siedel conjugate gradient iterative, 
EQ.14:  SSOR conjugate gradient iterative, 
EQ.15:  ILDLT0  (incomplete  factorization)  conjugate  gradient 
iterative, 
EQ.16:  modified  ILDLT0  (incomplete  factorization)  conjugate
gradient iterative. 
For Conjugate Heat transfer problems: 
EQ.17: GMRES solver. 
CGTOL 
Convergence tolerance for SOLVER = 3 and 4. 
EQ.0.0:  use default value 10−4 single or 10−6 double precision 
GPT 
Number of Gauss points to be used in the solid elements: 
EQ.0.0:  use default value 8, 
EQ.1.0:  one point quadrature is used. 
EQHEAT 
Mechanical equivalent of heat . 
EQ.0.0:  default value 1.0, 
LT.0.0:  designates  a  load  curve  number  for  EQHEAT  versus 
time. 
FWORK 
Fraction of mechanical work converted into heat. 
EQ.0.0:  use default value 1.0.
SBC 
*CONTROL_THERMAL_SOLVER 
DESCRIPTION
Stefan  Boltzmann  constant. 
radiation surfaces, see *BOUNDARY_RADIATION_… 
  Value  is  used  with  enclosure
LT.0.0:  use  a  smoothing  algorithm  when  calculating  view
factors to force the row sum = 1. 
MSGLVL 
Output message level  (For SOLVER > 10) 
EQ.0:  no output (default), 
EQ.1:  summary information, 
EQ.2:  detailed information, use only for debugging. 
MAXITR 
Maximum number of iterations.  For SOLVER > 11. 
EQ.0:  use default value 500, 
ABSTOL 
Absolute convergence tolerance.  For SOLVER > 11. 
EQ.0.0:  use default value 10−10 
RELTOL 
Relative 
SOLVER > 11. 
convergence 
tolerance. 
  Replaces  CGTOL 
for 
EQ.0.0:  use default value 10−6 
OMEGA 
Relaxation parameter omega for SOLVER 14 and 16. 
TSF 
EQ.0.0:  use default value 1.0 for Solver 14, use default value 0.0
for Solver 16. 
Thermal  Speedup  Factor.    This  factor  multiplies  all  thermal
parameters  with  units  of  time  in  the  denominator  (e.g.,  thermal
conductivity,  convection  heat  transfer  coefficients).    It  is  used  to
artificially  time  scale  the  problem.    Its  main  use  is  in  metal
stamping.    If  the  velocity  of  the  stamping  punch  is  artificially
increased  by  1000,  then  set  TSF = 1000  to  scale  the  thermal 
parameters. 
MXDMP 
Matrix Dumping for SOLVER > 11 
EQ.0:  No Dumping 
GT.0:  Dump using ASCII format every MXDMP time steps. 
LT.0:  Dump using binary format every |MXDMP| time steps.
DTVF 
Time interval between view factor updates.
VARIABLE   
VARDEN 
DESCRIPTION
Variable  thermal  density.    This  parameter  is  only  applicable  for
solid  elements  in  a  coupled  thermal-stress  problem.    Setting  this 
parameter will adjust the material thermal density in the thermal
solver  to  account  for  very  large  volume  changes  when  using  an 
EOS  or  large  coefficient  of  thermal  expansion. 
  For  most
applications, the default value, VARDEN = 0, should be used. 
EQ.0:  use constant density (default) 
EQ.1:  modify  thermal  density  to  account  for  volume  change
when using an EOS. 
EQ.2:  modify  thermal  density  to  account  for  volume  change 
when using a large coefficient of expansion. 
NINNER 
Number of inner iterations for GMRES solve 
NOUTER 
Number of outer iterations for GMRES solve 
Remarks: 
1.  Solver  Availability  in  MPP.    Solvers  1,  2,  3  and  4  are  only  for  SMP  environ-
ments.  Solvers 11, 12, 13, 14, 15 and 16 are for SMP and MPP. 
2.  Recommended Direct Solver.  Solver 11 is the preferred direct solver.  Solver 
11 uses sparse matrix storage and requires much less memory than Solver 1. 
3.  Direct vs.  Iterative Solve.  Use of a direct solver (e.g., SOLVER = 1, 2 or 11) is 
usually less efficient than using an iterative solver (SOLVER = 3, 4, 12, 13, 14, 15 
or 16).  Consider using a direct solver to get the model running and then switch 
to an iterative solver to decrease execution time (particularly for large models).  
Direct solvers should be used when experiencing slow or no convergence. 
4.  Transient  Problems.    For  transient  problems,  diagonal  scaling  conjugate 
gradient (SOLVER = 3 or 12) should be adequate. 
5.  Steady State Problems.  For steady state problems, convergence may be slow 
or unacceptable, so consider using direct solver (SOLVER = 1, 2 or 11) or a more 
powerful preconditioner (SOLVER = 4, 13, 14, 15 or 16). 
6.  Solvers 13 & 14.  Solver 13 (symmetric Gauss-Seidel) and solver 14 (SSOR) are 
related.  When OMEGA = 1, solver 14 is equivalent to solver 13.  The optimal 
omega value for SSOR is problem dependent but lies between 1 and 2.
7.  Solvers  15  &  16.    Solver  15  (incomplete  LDLT0)  and  solver  16  (modified 
incomplete LDLT0) are related.  Both are no-fill factorizations that require one 
extra n-vector of storage.  The sparsity pattern of the preconditioner is exactly 
the  same  as  that  of  the  thermal  stiffness  matrix.    Solver  16  uses  the  relaxation 
parameter OMEGA.  The optimal OMEGA value is problem dependent, but lies 
between 0 and 1. 
8.  Solver  17.    The  GMRES  solver  has  been  developed  as  an  alternative  to  the 
direct solvers in cases where the structural thermal problem is coupled with the 
fluid thermal problem in a monolithic approach using the ICFD solver.  A sig-
nificant gain of calculation time can be observed when the problem reaches 1M 
elements. 
9.  Completion  Conditions  for  Solvers  12  –  15.    Solvers  12,  13,  14,  15  and  16 
terminate  the  iterative  solution  process  when  (1)  the  number  of  iterations  ex-
ceeds MAXITR or (2) the 2-norm of the residual drops below 
ABSTOL  +  RELTOL × 2-norm of the initial residual. 
10.  Debug  Data.    Solvers  11  and  up  have  the  ability  to  dump  the  thermal 
conductance matrix and right-hand-side using the same formats as documented 
under  *CONTROL_IMPLICIT_SOLVER.    If  this  option  is  used  files  beginning 
with “T_”will be generated. 
11.  Unit  Conversion  Factor.    EQHEAT  is  a  unit  conversion  factor.    EQHEAT 
converts the mechanical unit for work into the thermal unit for energy accord-
ing to, 
EQHEAT × [work] = [thermal energy] 
However,  it  is  recommended  that  a  consistent  set  of  units  be  used  with 
EQHEAT set to 1.0.  For example  when using SI, 
[work] = 1Nm = [thermal energy] = 1J ⇒ EQHEAT = 1.
*CONTROL_THERMAL_TIMESTEP 
Purpose:    Set  time  step  controls  for  the  thermal  solution  in  a  thermal  only  or  coupled 
structural/thermal analysis.  This card requires that the deck also include *CONTROL_-
SOLUTION, and, *CONTROL_THERMAL_SOLVER needed. 
  Card 1 
Variable 
Type 
Default 
1 
TS 
I 
0 
2 
TIP 
3 
4 
5 
6 
7 
8 
ITS 
TMIN 
TMAX 
DTEMP 
TSCP 
LCTS 
F 
F 
0.5 
none 
F 
- 
F 
- 
F 
F 
1.0 
0.5 
I 
0 
  VARIABLE   
DESCRIPTION
TS 
Time step control: 
EQ.0: fixed time step, 
EQ.1: variable time step (may increase or decrease). 
TIP 
Time integration parameter: 
EQ.0.0: set to 0.5 - Crank-Nicholson scheme, 
EQ.1.0: fully implicit. 
ITS 
Initial thermal time step 
TMIN 
Minimum thermal time step: 
EQ.0.0: set to structural explicit time step. 
TMAX 
Maximum thermal time step: 
EQ.0.0: set to 100 * structural explicit time step. 
DTEMP 
Maximum temperature change in each time step above which the
thermal time step will be decreased: 
EQ.0.0: set to a temperature change of 1.0. 
TSCP 
Time step control parameter.  The thermal time step is decreased
by this factor if convergence is not obtained.  0. < TSCP < 1.0: 
EQ.0.0: set to a factor of 0.5.
LCTS 
*CONTROL_THERMAL_TIMESTEP 
DESCRIPTION
LCTS designates a load curve number which defines data pairs of
(thermal  time  breakpoint,  new  time  step).    The  time  step  will  be
adjusted  to  hit  the  time  breakpoints  exactly.    After  the  time
breakpoint,  the  time  step  will  be  set  to  the  ‘new  time  step’
ordinate value in the load curve.
*CONTROL 
Purpose:  Set structural time step size control using different options. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DTINIT 
TSSFAC 
ISDO 
TSLIMT 
DT2MS 
LCTM 
ERODE 
MS1ST 
Type 
F 
F 
Default 
- 
0.9 or 
0.67 
I 
0 
F 
F 
0.0 
0.0 
I 
0 
I 
0 
I 
0 
This card is optional. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DT2MSF  DT2MSLC 
IMSCL 
RMSCL 
Type 
F 
I 
Default 
not 
used 
not 
used 
I 
0 
F 
0.0 
  VARIABLE   
DESCRIPTION
DTINIT 
Initial time step size: 
EQ.0.0: LS-DYNA determines initial step size. 
TSSFAC 
Scale  factor  for  computed  time  step  (old  name  SCFT).    See
Remark 1 below.  (Default = 0.90; if high explosives are used, the 
default is lowered to 0.67).
ISDO 
*CONTROL_TIMESTEP 
DESCRIPTION
Basis  of  time  size  calculation  for  4-node  shell  elements.    3-node 
shells  use  the  shortest  altitude  for  options  0,1  and  the  shortest
side for option 2.  This option has no relevance to solid elements,
which use a length based on the element volume divided by the 
largest surface area. 
EQ.0: characteristic length is given by 
area
min(longest side,  longest diagonal )
. 
EQ.1: characteristic length is given by 
area
longest diagonal
. 
EQ.2: based on bar wave speed and, 
max [shortest side,
area
min(longest side,  longest diagonal )
]  . 
WARNING:  Option 2 can give a much larger time 
step  size  that  can  lead  to  instabilities 
in some applications, especially when 
triangular elements are used. 
EQ.3: This  feature  is  currently  unavailable.    Time  step  size  is
based on the maximum eigenvalue.  This option is okay 
for  structural  applications  where  the  material  sound
speed  changes  slowly.    The  cost  related  to  determining
the  maximum  eigenvalue  is  significant,  but  the  increase
in the time step size often allows for significantly shorter
run times without using mass scaling.
VARIABLE   
TSLIMT 
DESCRIPTION
Shell element minimum time step assignment, TSLIMT.  When a
shell  controls  the  time  step,  element  material  properties  (moduli
not masses) will be modified such that the time step does not fall
below  the  assigned  step  size.    This  option  is  applicable  only  to
shell elements using material models: 
*MAT_PLASTIC_KINEMATIC,  
*MAT_POWER_LAW_PLASTICITY, 
*MAT_STRAIN_RATE_DEPENDENT_PLASTICITY, 
*MAT_PIECE-WISE_LINEAR_PLASTICITY. 
WARNING:  This so-called stiffness scaling option is 
NOT  recommended.    The  DT2MS  op-
tion  below  applies  to  all  materials  and 
element classes and is preferred. 
If  both  TSLIMT  and  DT2MS  below  are  active  and  if  TSLIMT  is 
input  as  a  positive  number,  then  TSLIMT  defaults  to  10−18, 
thereby disabling it. 
If TSLIMT is negative and less than |DT2MS|, then |TSLIMT| is
applied prior to the mass being scaled.  If |DT2MS| exceeds the
magnitude of TSLIMT, then TSLIMT is set to 10−18.
VARIABLE   
DESCRIPTION
DT2MS 
Time step size for mass scaled solutions.  (Default = 0.0) 
GT.0.0: Positive  values  are  for  quasi-static  analyses  or  time 
history analyses where the inertial effects are insignifi-
cant. 
LT.0.0:  TSSFAC × |DT2MS|  is  the  minimum  time  step  size 
permitted  and  mass  scaling  is  done  if  and  only  if  it  is
necessary  to  meet  the Courant time  step  size  criterion.
This    option  can  be  used  in  transient  analyses  if  the
mass increases remain insignificant.  See also the varia-
ble  MS1ST  below  and  the  *CONTROL_TERMINA-
TION variable ENDMAS. 
WARNING: 
Superelements  from,  *ELEMENT_DI-
RECT_MATRIX_INPUT, are not mass 
scaled;  consequently,  DT2MS  does 
not affect their time step size.  In this 
case  an  error  termination  will  occur, 
and DT2MS will need to be reset to a 
smaller value. 
LCTM 
Load curve ID that limits the maximum time step size (optional).
This  load  curve  defines  the  maximum  time  step  size  permitted
versus  time.    If  the  solution  time  exceeds  the  final  time  value
defined by the curve the computed step size is used.  If the time
step  size  from  the  load  curve  is  exactly  zero,  the  computed  time
step size is also used.
VARIABLE   
DESCRIPTION
ERODE 
Erosion flag for solids and thick shells.  
EQ.0: Calculation  will  terminate  if  time  step  drops  to  tsmin 
. 
EQ.1: Solids  and  thick  shells  whose  time  step  drops  to    tsmin
  will  erode,  and  SPH 
particles  whose  time  step  drops  to    tsmin  will  be  deac-
tivated. 
ERODE = 1  and  tsmin > 0  also  invokes  erosion  of  any  solid 
element  whose  volume  becomes  negative,  thereby  preventing
termination of the analysis due to negative volume.  The effect of
ERODE = 1  on  erosion  due  to  negative  volue  is  superceded  by  a
nonzero  PSFAIL  in  *CONTROL_SOLID.    PSFAIL  serves  to  limit 
solid erosion based on negative volume to  solids in part set PS-
FAIL.  
MS1ST 
Option for mass scaling that applies when DT2MS < 0. 
EQ.0: (Default)  Mass  scaling  is  considered  throughout  the
analysis  to  ensure  that  the  minimum  time  step  cannot 
drop  below  TSSFAC × |DT2MS|.    Added  mass  may  in-
crease with time, but it will never decrease.  
EQ.1: Added  mass  is  calculated  at  the  first  time  step  and
remains unchanged thereafter.  The initial time step will
not  be  less  than  TSSFAC × |DT2MS|,  but  the  time  step 
may subsequently decrease, depending on how the mesh
deforms and the element characteristic lengths change. 
DT2MSF 
Reduction  (or  scale)  factor  for  initial  time  step  size  to  determine
the minimum time step size permitted.  Mass scaling is done if it 
is  necessary  to  meet  the  Courant  time  step  size  criterion.    If  this
option is used, DT2MS effectively becomes  –DT2MSF multiplied 
by  the  initial  time  step  size,  Δ𝑡,  before  Δ𝑡  is  scaled  by  TSSFAC. 
This option is active if and only if DT2MS = 0 above.
DT2MSLC 
*CONTROL_TIMESTEP 
DESCRIPTION
Load  curve  for  determining  the  magnitude  of  DT2MS  as  a
function  of  time,  𝑓DT2MS(𝑡),  during  the  explicit  solutions  phase. 
Time  zero  must  be  in  the  abscissa  range  of  this  curve  and  the 
ordinate values should all be positive.  At a given simulation time
𝑡, 𝑓DT2MS(𝑡) × sign(DT2MS) plays the role of DT2MS according to 
the description for DT2MS above.  It is allowed to use all negative 
ordinate  values  in  the  curve,  then  𝑓DT2MS(𝑡)  itself  (sign  and 
magnitude)  determines  how  mass  scaling  is  performed  and
DT2MS  is  neglected.    It  is  however  not  allowed  for  the  ordinate 
values to change sign during the simulation. 
IMSCL 
Flag  for  selective  mass  scaling  if  and  only  if  mass  scaling  active. 
Selective  mass  scaling  does  not  scale  the  rigid  body  mass  and  is
therefore more accurate.  Since it is memory and CPU intensive, it
should be applied only to small finely meshed parts.   
EQ.0: no selective mass scaling. 
EQ.1: all parts undergo selective mass scaling. 
LT.0:  recommended: 
|IMSCL| is the part set ID of the parts 
that  undergo  selective  mass  scaling;  all  other  parts  are
mass scaled the usual way. 
RMSCL 
Flag for using rotational option in selective mass scaling 
EQ.0.: Only translational inertia are selectively mass scaled 
NE.0.:  Both  translational  and  rotational  inertia  are  selectively
mass scaled 
Remarks: 
During the solution we loop through the elements and determine a new time step size 
by taking the minimum value over all elements. 
Δ𝑡 𝑛+1 = TSSFAC × min{Δ𝑡1, Δ𝑡2, . . . , Δ𝑡𝑁} 
where  N    is  the  number  of  elements.    The  time  step  size  roughly  corresponds  to  the 
transient time of an acoustic wave through an element using the shortest characteristic 
distance.  For stability reasons the scale factor TSSFAC is typically set to a value of 0.90 
(default) or some smaller value.  To decrease solution time we desire to use the largest 
possible  stable  time  step  size.    Values  larger  than  .90  will  often  lead  to  instabilities.  
Some comments follow:
1.  Sound Speed and Element Size.  The sound speed in steel and aluminum is 
approximately 5mm per microsecond; therefore, if a steel structure is modeled 
with element sizes of 5mm, the computed time step size would be 1 microsec-
ond.  Elements made from materials with lower sound speeds, such as  foams, 
will give larger time step sizes.  Avoid excessively small elements and be aware 
of  the  effect  of  rotational  inertia  on  the  time  step  size  in  the  Belytschko  beam 
element.  Sound speeds differ for each material, for example, consider: 
Air 
Water 
Steel 
Titanium 
Plexiglass 
331  m/s 
1478 
5240 
5220 
2598 
2.  Use Rigid Bodies when Possible.  It is recommended that stiff components be 
modeled by using rigid bodies.  Do not scale the Young’s modulus, as that can 
substantially reduce the time step size. 
3.  Triangular Elements.  The altitude of the triangular element should be used to 
compute the time step size.  Using the shortest side is okay only if the calcula-
tion is closely examined for possible instabilities.  This is controlled by parame-
ter ISDO. 
4.  Selective  Mass  Scaling.    In  the  explicit  time  integration  context  and  in 
contrast  to  conventional  mass  scaling,  selective  mass  scaling  (SMS)  is  a  well 
thought out scheme that not only reduces the number of simulation cycles but 
that also does not significantly affect the dynamic response of the system under 
consideration.    The  drawback  is  that  a  linear  system  of  equations  must  be 
solved  in  each  time  step  for  the  accelerations.      In  this  implementation  a  pre-
conditioned conjugate gradient method (PCG) is used. 
An  unfortunate  consequence  of  this  choice  of  solver  is  that  the  efficiency  will 
worsen  when  attempting  large  time  steps  since  the  condition  number  of  the 
assembled  mass  matrix  increases  with  the  added  mass.    Therefore  caution 
should be taken when choosing the desired time step size.  For large models it 
is also recommended to only use SMS on critical parts since it is otherwise like-
ly  to  slow  down  execution;    the  bottleneck being  the  solution  step  for the  sys-
tem of linear system of equations. 
While some constraints and boundary conditions available in LS-DYNA are not 
supported for SMS they can be implemented upon request from a user. 
A partial list of constraints and boundary conditions supported with SMS: 
Pointwise nodal constraints in global and local directions 
Prescribed motion in global and local directions
Adaptivity 
Rigid walls 
Deformable elements merged with rigid bodies 
Constraint contacts and spotwelds 
Beam release constraints 
By  default,  only  the  translational  dynamic  properties  are  treated.    This  means 
that only rigid body translation will be unaffected by the mass scaling imposed.  
There is an option to also properly treat rigid body rotation in this way, this is 
invoked  by  flagging  the  parameter  RMSCL.    A  penalty  in  computational  ex-
pense is incurred but the results could be improved if rotations are dominating 
the simulation.
*CONTROL 
Purpose:  Specify  the  user  units  for  the  current  keyword  input  deck.    This  does  not 
provide any mechanism for automatic conversion of units of any entry in the keyword 
input  deck.    It  is  intended  to  be  used  for  several  purposes,  but  currently  only  for  the 
situation where an external database in another set of units will be loaded and used in 
the simulation.  In this case, *CONTROL_UNITS provides the information necessary to 
convert  the  external  data  into  internal  units  . 
If the needed unit is not one of the predefined ones listed for use on the first card, then 
the  second  optional  card  is  used  to  define  that  unit.    Any  non-zero  scales  that  are 
entered on optional card 2 override what is specified on the first card.  These scales are 
given  in  terms  of  the  default  units  on  card  1.    For  instance,  if  3600.0  is  given  in  the 
second 20 character field on the optional second card (TIME_SCALE), then ‘hour’ is the 
time unit (3600 seconds). 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LENGTH 
TIME 
MASS 
TEMP 
Type 
A 
A 
A 
Default 
m 
sec 
kg 
A 
K 
Optional Card only used when a new unit needs to be defined:  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LENGTH_SCALE 
TIME_SCALE 
MASS_SCALE 
Type 
F 
Default 
1.0 
F 
1.0 
F 
1.0
VARIABLE   
DESCRIPTION
LENGTH 
Length units: 
EQ.m:  meter (default)  
EQ.mm:  millimeter 
EQ.cm:  centimeter 
EQ.in: 
inch 
EQ.ft: 
foot 
TIME 
Time units: 
EQ.sec: 
EQ.ms: 
second (default) 
msec, millisec 
EQ.micro_s:  microsec 
MASS 
Mass units: 
EQ.kg: 
EQ.g: 
EQ.mg: 
EQ.lb: 
kilogram (default) 
gram 
milligram 
pound 
EQ.slug: 
pound × sec2/foot 
EQ.slinch: 
pound × sec2/inch 
EQ.mtrc_ton:  metric_ton 
TEMP 
Temperature units: 
EQ.K:  Kelvin (default) 
EQ.C:  Celsius 
EQ.F:  Fahrenheit 
EQ.R:  Rankine 
LENGTH_
SCALE 
TIME_
SCALE 
MASS_
SCALE 
Number of meters in the length unit for the input deck 
Number of seconds in the time unit for the input deck 
Number of kilograms in the mass unit for the input deck
The Keyword options in this section in alphabetical order are: 
*DAMPING_FREQUENCY_RANGE_{OPTION} 
*DAMPING_GLOBAL 
*DAMPING_PART_MASS 
*DAMPING_PART_STIFFNESS 
*DAMPING_RELATIVE
*DAMPING_FREQUENCY_RANGE_{OPTION} 
Purpose:    This  feature  provides  approximately  constant  damping  (i.e.    frequency-
independent) over a range of frequencies. 
Available OPTIONS are: 
<BLANK>  Applies damping to global motion 
DEFORM  Applies damping to element deformation 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CDAMP 
FLOW 
FHIGH 
PSID 
(blank) 
PIDREL 
IFLG 
Type 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
CDAMP 
Damping in fraction of critical. 
FLOW 
FHIGH 
PSID 
PIDREL 
Lowest  frequency  in  range  of  interest  (cycles  per  unit  time,  e.g.
Hz if time unit is seconds) 
Highest  frequency  in  range  of  interest  (cycles  per  unit  time,  e.g.
Hz if time unit is seconds) 
Part set ID.  The requested damping is applied only to the parts in 
the  set.    If  PSID = 0,  the  damping  is  applied  to  all  parts  except
those  referred  to  by  other  *DAMPING_FREQUENCY_RANGE 
cards. 
Optional  part  ID  of  rigid  body.    Damping  is  then  applied  to  the
motion  relative  to  the  rigid  body  motion.    This  input  does  not 
apply to the DEFORM option. 
IFLG 
Method used for internal calculation of damping constants:  
EQ.0:  Iterative (more accurate), 
EQ.1:  Approximate (same as R9 and previous versions).
Remarks: 
This  feature  provides  approximately  constant  damping  (i.e.    frequency-independent) 
over  a  range  of  frequencies.  𝐹low < 𝐹 < 𝐹highIt  is  intended  for  small  damping  ratios 
(e.g. < 0.05)  and  frequency  ranges  such  that  𝐹high/𝐹low  is  in  the  range  10  to  300.    The 
drawback  to  this  method  of  damping  is  that  it  reduces  the  dynamic  stiffness  of  the 
model, especially at low frequencies. 
Where  the  model  contains,  for  example,  a  rigid  foundation  or  base,  the  effects  of  this 
stiffness  reduction  can  be  ameliorated  by  using  PIDREL.    In  this  case,  the  damping 
forces  resist  motion  relative  to  the  base,  and  are  reacted  onto  the  rigid  part  PIDREL.  
“Relative  motion”  here  means  the  difference  between  the  velocity  of  the  node  being 
damped,  and  the  velocity  of  a  point  rigidly  connected  to  PIDREL  at  the  same 
coordinates as the node being damped. 
This effect is predictable: the natural frequencies of modes close to 𝐹low are reduced by 
3% for a damping ratio of 0.01 and 𝐹high/𝐹low in the range 10-30.  Near 𝐹high the error is 
between zero and one third of the error at 𝐹low.  Estimated frequency errors are shown 
in the next table. 
Damping 
Ratio 
0.01 
0.02 
0.04 
% error for Fhigh/Flow  =  
3 to 30 
30 to 300 
300 to 3000 
3%  
6% 
12% 
4.5% 
9% 
18% 
6% 
12% 
24% 
It  is  recommended  that  the  elastic  stiffnesses  in  the  model  be  increased  slightly  to 
account  for  this,  e.g.    for  0.01  damping  across  a  frequency  range  of  30  to  600Hz,  the 
average error across the frequency range is about 2%.  Increase the stiffness by (1.02)2, 
i.e.  by 4%. 
Starting  from  R10,  an  iterative  method  is  used  for  the  internal  calculation  of  the 
damping  constants  .    The  new  method  results  in  the  actual  damping 
matching  the  user-input  damping  ratio  CDAMP  more  closely  across  the  frequency 
range  FLOW  to  FHIGH.    As  an  example,  for  CDAMP = 0.01,  FLOW = 1  Hz  and 
FHIGH = 30  Hz,  the  actual  damping  achieved  by  the  previous  approximate  method 
varied  between  0.008  and  0.012  (different  values  at  different  frequencies),  i.e.    there 
were errors of up to 20% of the target CDAMP.  With the iterative algoritm, the errors 
are reduced to 1% of the target CDAMP.
*DAMPING_FREQUENCY_RANGE 
The  DEFORM  option  applies  damping  to  the  element  responses  (unlike  the  standard 
*DAMPING_FREQUENCY_RANGE  which  damps  the  global  motion  of  the  nodes).  
Therefore,  rigid  body  motion  is  not  damped  when  the  DEFORM  keyword  option  is 
used.    For  this  reason,  DEFORM  is  recommended  over  the  standard  option.    The 
damping  is  adjusted  based  on  current  tangent  stiffness;  this  is  believed  to  be  more 
appropriate  for  a  nonlinear  analysis,  which  could  be  over-damped  if  a  strain-rate-
proportional or viscous damping scheme were used.   
It works with the following element formulations: 
•  Solids – types -1, -2, 1, 2, 3, 4, 9, 10, 13, 15, 16, 17, 99 
•  Beams – types 1, 2, 3, 4, 5, 9 (note: not type 6) 
•  Shells – types 1-5, 7-17, 20, 21, 23-27, 99 
•  Discrete elements 
The DEFORM option differs from the standard option in several ways: 
Standard Damping vs.  Deformation Damping 
Characteristic 
Property 
Keyword Option 
<BLANK> 
DEFORM 
Damping on 
Node velocities 
Element responses 
Rigid body motion 
Can be damped 
Never damped 
Natural frequencies 
Reduced (by percentages 
shown in the above table) 
Increased (percentages shown 
in the above table) 
Recommended 
compensation 
Increase elastic stiffness 
Reduce elastic stiffness 
Effect on timestep 
None 
Small reduction applied 
automatically, same 
percentage as in the frequency 
change 
Element types 
damped 
All 
See list above 
Damping energy 
output 
Included in “system damping 
energy” 
Included in Internal Energy 
only if RYLEN = 2 on *CON-
TROL_ENERGY
*DAMPING 
Purpose:    Define  mass  weighted  nodal  damping  that  applies  globally  to  the  nodes  of 
deformable bodies and to the mass center of the rigid bodies.  For specification of mass 
damping by part ID or part set ID, use *DAMPING_PART_MASS. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
VALDMP 
STX 
STY 
STZ 
SRX 
SRY 
SRZ 
Type 
Default 
Remarks 
I 
0 
1 
  VARIABLE   
LCID 
F 
F 
F 
F 
F 
F 
F 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
2 
2 
2 
2 
2 
2 
DESCRIPTION
Load curve ID  which specifies the system 
damping constant vs.  time: 
EQ.0:  a  constant  damping  factor  as  defined  by  VALDMP  is
used, 
GT.0:  system  damping  is  given  by  load  curve  LCID  (which
must be an integer).  The damping force applied to each
node is 𝑓 = −𝑑(𝑡)𝑚𝑣, where 𝑑(𝑡) is defined by load curve 
LCID. 
VALDMP 
System damping constant, Ds (this option is bypassed if the load 
curve number defined above is non zero). 
STX 
STY 
STZ 
SRX 
SRY 
SRZ 
Scale factor on global 𝑥 translational damping forces. 
Scale factor on global 𝑦 translational damping forces. 
Scale factor on global 𝑧 translational damping forces. 
Scale factor on global 𝑥 rotational damping moments. 
Scale factor on global 𝑦 rotational damping moments. 
Scale factor on global 𝑧 rotational damping moments.
*DAMPING_GLOBAL 
1.  Restart.  This keyword is also used for the restart, see *RESTART. 
2.  Defaults  for  Scale  Factors.    If  STX  = STY = STZ  = SRX  = SRY = SRZ  = 0.0  in 
the input above, all six values are defaulted to unity. 
3.  Damping Exceptions.  Mass damping will not be applied to deformable nodes 
with prescribed motion or to nodes tied with CONSTRAINED_NODE_SET. 
4.  Formulation.    With  mass  proportional  system  damping  the  acceleration  is 
computed as: 
𝐚𝑛 = 𝐌−1(𝐏𝑛 − 𝐅𝑛 − 𝐅damp
where, 𝐌 is the diagonal mass matrix, 𝐏𝐧 is the  external load vector, 𝐅𝑛 is the 
internal load vector, and 𝐅damp
 is the force vector due to system damping.  This 
latter vector is defined as: 
) 
𝐅damp
= 𝐷𝑠𝑚𝐯 
The  best  damping  constant  for  the  system  is  usually  some  value  approaching 
the critical damping factor for the lowest frequency mode of interest. 
(𝐷𝑠)critical = 2𝜔min 
The natural frequency 𝜔min (given in radians per unit time) is generally taken as 
the fundamental frequency of the structure.  This frequency can be determined 
from an eigenvalue analysis or from an undamped transient analysis.  Note that 
this  damping  applies  to  both  translational  and  rotational  degrees  of  freedom.  
Also note that mass proportional damping will damp rigid body motion as well 
as vibration. 
Energy  dissipated  by  through  mass  weighted  damping  is  reported  as  system 
damping  energy  in  the  ASCII  file  glstat.    This  energy  is  computed  whenever 
system damping is active.
*DAMPING 
OPTION specifies that a part set ID is given with the single option: 
<BLANK> 
SET 
If not used a part ID is assumed. 
Purpose:    Define  mass  weighted  damping  by  part  ID.    Parts  may  be  either  rigid  or 
deformable.  In rigid bodies the damping forces and moments act at the center of mass.  
This  command  may  appear  multiple  times  in  an  input  deck  but  cannot  be  combined 
with *DAMPING_GLOBAL. 
  Card 1 
1 
2 
Variable 
PID/PSID 
LCID 
Type 
Default 
I 
0 
I 
0 
3 
SF 
F 
1.0 
4 
5 
6 
7 
8 
FLAG 
I 
0 
Scale Factor Card.  Additional Card for FLAG = 1.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
STX 
STY 
STZ 
SRX 
SRY 
SRZ 
Type 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
PID/PSID 
Part ID, see *PART or part set ID, see *SET_PART. 
LCID 
Load  curve  ID    which  specifies  the 
damping  constant  vs.    time,  applied  to  the  part(s)  specified  in
PID/PSID.
VARIABLE   
DESCRIPTION
Scale factor for load curve.  This allows a simple modification of
the load curve values. 
Set  this  flag  to  unity  if  the  global  components  of  the  damping 
forces require separate scale factors. 
Scale factor on global 𝑥 translational damping forces. 
Scale factor on global 𝑦 translational damping forces. 
Scale factor on global 𝑧 translational damping forces. 
Scale factor on global 𝑥 rotational damping moments. 
Scale factor on global 𝑦 rotational damping moments. 
Scale factor on global 𝑧 rotational damping moments. 
SF 
FLAG 
STX 
STY 
STZ 
SRX 
SRY 
SRZ 
Remarks: 
Mass  weighted  damping  damps  all  motions  including  rigid  body  motions.    For  high 
frequency oscillatory motion stiffness weighted damping may be preferred.  With mass 
proportional system damping the acceleration is computed as: 
𝛂𝑛 = 𝐌−1(𝐏𝑛 − 𝐅𝑛 − 𝐅damp
where, 𝐌 is the diagonal mass matrix, 𝐏𝑛 is the external load vector, 𝐅𝑛 is the internal 
 is the force vector due to system damping.  This latter vector is 
load vector, and 𝐅damp
defined as: 
) 
𝐅damp
= 𝐷𝑠𝑚𝝂 
The critical damping constant for the lowest frequency mode of interest is   
𝐷𝑠 = 2𝜔min 
where  𝜔min  is  that  lowest  frequency  in  units  of  radians  per  unit  time.    The  damping 
constant  specified  as  the  ordinate  of  curve  LCID  is  typically  less  than  the  critical 
damping constant.  The damping is applied to both translational and rotational degrees 
of freedom.  The component scale factors can be used to limit which global components 
see damping forces. 
Energy dissipated by through mass weighted damping is reported as system damping 
energy in the ASCII file glstat.  This energy is computed whenever system damping is 
active.
Mass  damping  will  not  be  applied  to  deformable  nodes  with  prescribed  motion  or  to 
nodes tied with CONSTRAINED_NODE_SET.
*DAMPING_PART_STIFFNESS_{OPTION} 
OPTION specifies that a part set ID is given with the single option: 
<BLANK> 
SET 
If the SET option is not used, a part ID goes in the first field of Card 1. 
Purpose:  Assign Rayleigh stiffness damping coefficient by part ID or part set ID.   This 
damping  command  does  not  apply  to  parts  comprised  of  discrete  elements  (*ELE-
MENT_DISCRETE) or discrete beams (*ELEMENT_BEAM with ELFORM = 6).  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID/PSID 
COEF 
Type 
I 
F 
Default 
none 
0.0 
  VARIABLE   
DESCRIPTION
PID/PSID 
Part ID  or part set ID . 
COEF 
Rayleigh damping coefficient.  Two methods are now available: 
LT.0.0:  Rayleigh damping coefficient in units of time, set based
on a given frequency and applied uniformly to each el-
ement in the specified part or part set.  See remarks be-
low. 
EQ.0.0:  Inactive. 
GT.0.0:  Rayleigh  damping  coefficient  for  stiffness  weighted
damping.    Values  between  0.01  and  0.25  are  recom-
mended.  Higher values are strongly discouraged, and
values less than 0.01 may have little effect.  The damp-
ing  coefficient  is  uniquely  defined  for  each  element  of
the part ID. 
Remarks: 
The damping matrix in Rayleigh damping is defined as:
𝐂 = 𝛼𝐌 + 𝛽𝐊 
where  𝐂,  𝐌,  and  𝐊  are  the  damping,  mass,  and  stiffness  matrices,  respectively.    The 
constants  α.    and  β  are  the  mass  and  stiffness  proportional  damping  constants.    The 
mass proportional damping can be treated by system damping, see keywords: *DAMP-
ING_GLOBAL and DAMPING_PART_MASS.  Transforming 𝐂 with the ith eigenvector 
𝛟𝑖 gives: 
𝛟𝑖
T𝐂𝛟𝑖 = 𝛟𝑖
T(𝛼𝐌 + 𝛽𝐊)𝛟𝑖 = 𝛼 + 𝛽𝜔𝑖
2 = 2𝜔𝑖𝜉𝑖𝛿𝑖𝑗 
where  𝜔𝑖  is  the  ith  frequency  (radians/unit  time)  and  𝜉𝑖  is  the  corresponding  modal 
damping parameter. 
Generally,  the  stiffness  proportional  damping  is  effective  for  high  frequencies  and  is 
orthogonal to rigid body motion.  Mass proportional damping is more effective for low 
frequencies  and  will  damp  rigid  body  motion.    If  a  large  value  of  the  stiffness  based 
damping  coefficient  is  used,  it  may  be  necessary  to  lower  the  time  step  size 
significantly.  This must be done manually by reducing the time step scale factor on the 
*CONTROL_TIMESTEP  control  card.    Since  a  good  value  of  β  is  not  easily  identified, 
the  coefficient,  COEF,  is  defined  such  that  a  value  of  .10  roughly  corresponds  to  10% 
damping in the high frequency domain. 
In  LS-DYNA  versions  prior  to  960  or  if  COEF  is  input  as  less  than  0,  the  critical 
damping coefficient is equal to 2 divided by 𝜔𝑖.  For example, 10% of critical damping 
in the ith mode corresponds to  
𝛽 =
0.20
𝜔𝑖
and COEF would be input as -𝛽.  Typically, this method of applying stiffness damping 
is stable only if 𝛽 is significantly smaller than the explicit time step size.   
Energy dissipated by Rayleigh damping is computed if and only if the flag, RYLEN, on 
the  control  card,  *CONTROL_ENERGY  is  set  to  2.    This  energy  is  accumulated  as 
element  internal  energy  and  is  included  in  the  energy  balance.    In  the  glstat  file  this 
energy will be lumped in with the internal energy. 
NOTE: Type 2 beam elements are a special case in which COEF is internally scaled by 
0.1.  Thus there is a factor of 10 less damping than stated above.   This applies to both 
negative and positive values of COEF.
*DAMPING_RELATIVE 
Purpose:  Apply damping relative to the motion of a rigid body.  For example, it could 
damp  the  deformation  of  a  rotating  tire  relative  to  the  wheel  without  damping  the 
rotating motion. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CDAMP 
FREQ 
PIDRB 
PSID 
DV2 
LCID 
Type 
Default 
F 
0 
F 
0 
F 
0 
I 
0 
F 
0.0 
I 
0 
  VARIABLE   
DESCRIPTION
CDAMP 
Fraction of critical damping. 
Frequency at which CDAMP is to apply (cycles per unit time, e.g.
Hz if time unit is seconds). 
Part  ID  of  rigid  body,  see  *PART.    Motion  relative  to  this  rigid
body will be damped. 
Part set ID.  The requested damping is applied only to the parts in
the set. 
Optional constant for velocity-squared term.  See remarks. 
ID  of  curve  that  defines  fraction  of  critical  damping  vs.    time.
CDAMP will be ignored if LCID is non-zero. 
FREQ 
PIDRB 
PSID 
DV2 
LCID 
Remarks: 
1.  This  feature  provides  damping  of  vibrations  for  objects  that  are  moving 
through space.  The vibrations are damped, but not the rigid body motion.  This 
is  achieved  by  calculating  the  velocity  of  each  node  relative  to  that  of  a  rigid 
body,  and  applying  a  damping  force  proportional  to  that velocity.    The  forces 
are reacted onto the rigid body such that overall momentum is conserved.  It is 
intended that the rigid body is embedded within the moving object. 
2.  Vibrations  at  frequencies  below  FREQ  are  damped  by  more  than  CDAMP, 
while those at frequencies above FREQ are damped by less than CDAMP.  It is
recommended  that  FREQ  be  set to the  frequency  of  the  lowest  mode  of  vibra-
tion. 
3.  The damping force of each node is calculated as follows: 
 F = - (D .  m .  v) – (DV2 .  m .v2).    
Where: 
D = 4π .  CDAMP .  FREQ 
m =  mass of the node 
v = velocity  of  node  relative  to  the  velocity  of  a  point  on  the  rigid 
body at the same coordinates as the node.
The database definitions are optional, but are necessary to obtain output files containing 
results  information.    In  this  section  the  database  keywords  are  defined  in  alphabetical 
order: 
*DATABASE_OPTION 
*DATABASE_ALE 
*DATABASE_ALE_MAT 
*DATABASE_BINARY_OPTION 
*DATABASE_BINARY_D3PROP 
*DATABASE_CPM_SENSOR 
*DATABASE_CROSS_SECTION_OPTION1_{OPTION2} 
*DATABASE_EXTENT_OPTION 
*DATABASE_FATXML 
*DATABASE_FORMAT 
*DATABASE_FREQUENCY_ASCII_OPTION 
*DATABASE_FREQUENCY_BINARY_OPTION 
*DATABASE_FSI 
*DATABASE_FSI_SENSOR 
*DATABASE_HISTORY_OPTION 
*DATABASE_MASSOUT 
*DATABASE_NODAL_FORCE_GROUP 
*DATABASE_PROFILE 
*DATABASE_PAP_OUTPUT 
*DATABASE_PWP_FLOW 
*DATABASE_PWP_OUTPUT
*DATABASE_RECOVER_NODE 
*DATABASE_SPRING_FORWARD 
*DATABASE_SUPERPLASTIC_FORMING 
*DATABASE_TRACER 
*DATABASE_TRACER_GENERATE 
The ordering of the database definition cards in the input file is completely arbitrary.
*DATABASE 
OPTION1  specifies  the  type  of  database.    LS-DYNA  will not  create  an  ASCII  database 
unless  the  corresponding  *DATABASE_OPTION1  card  is  included  in  the  input  deck.  
OPTION1 may be any of the items in the following list: 
ABSTAT  Airbag statistics. 
ATDOUT  Automatic  tiebreak  damage  statistics  for  *CONTACT_AUTOMAT-
IC_ONE_WAY_SURFACE_TO_SURFACE_TIEBREAK,  OPTIONs  7, 
9, 10, and 11 (only SMP at the moment). 
AVSFLT  AVS database.  See *DATABASE_EXTENT_OPTION. 
BEARING 
*ELEMENT_BEARING force output. 
BNDOUT 
Boundary condition forces and energy  
CURVOUT  Output from *DEFINE_CURVE_FUNCTION.  
DEFGEO  Deformed  geometry  file.    (Note  that  to  output  this  file  in  Chrysler 
format  insert  the  following  line  in  your  .cshrc  file:  “setenv  LSTC_
DEFGEO chrysler”)  The nasbdf file (NASTRAN Bulk Data) is creat-
ed whenever the DEFGEO file is requested. 
DCFAIL 
Failure function data for *MAT_SPOTWELD_DAIMLERCHRYSLER 
DEFORC  Discrete  spring  and  damper  element  (*ELEMENT_DISCRETE)  data.  
If  the  user  wishes  to  be  selective  about  which  discrete  elements  are 
output  in  deforc,  use  *DATABASE_HISTORY_DISCRETE_OPTION 
to  select  elements  for    output  (but  only  if  BEAM = 0  in  *DATA-
BASE_BINARY_D3PLOT) or set PF = 1 in *ELEMENT_DISCRETE to 
turn  off  output  for  particular  elements;  otherwise  all  discrete  ele-
ments are output. 
DEMASSFLOW  Measure  mass  flow  rate  across  defined  plane  and  use  together  with 
*DEFINE_DE_MASSFLOW_PLANE. 
DISBOUT  Discrete beam element, type 6, relative displacements, rotations, and 
force resultants, all in the local coordinate system, which is also out-
put.  Use with *DATABASE_HISTORY_BEAM. 
ELOUT 
Element data.  See *DATABASE_HISTORY_OPTION.  Also, see Card 
3  of  the  *DATABASE_EXTENT_BINARY  parameters  INTOUT  and 
NODOUT.  This latter option will output all integration point data or 
extrapolated data to the connectivity nodes in a file call eloutdet. 
GCEOUT  Geometric contact entities. 
GLSTAT  Global data.  Always obtained if ssstat file is activated. 
H3OUT  Hybrid III rigid body dummies. 
JNTFORC 
Joint force file
MATSUM  Material energies.  See Remarks 1 and 2 below. 
MOVIE 
MPGS 
See MOVIE option of *DATABASE_EXTENT_OPTION. 
See MPGS option of *DATABASE_EXTENT_OPTION. 
NCFORC  Nodal interface forces.  See *CONTACT - Card 1 (SPR and MPR) 
NODFOR  Nodal force groups.  See *DATABASE_NODAL_FORCE_GROUP. 
NODOUT  Nodal point data.  See *DATABASE_HISTORY_NODE_OPTION. 
PBSTAT 
Particle blast data.  See *PARTICLE_BLAST 
PLLYOUT 
Pulley element data for *ELEMENT_BEAM_PULLEY. 
PRTUBE 
Pressure tube data for *DEFINE_PRESSURE_TUBE. 
RBDOUT  Rigid body data.  See Remark 2 below. 
RCFORC  Resultant  interface  forces.    Output  in  a  local  coordinate  system  is 
available, see *CONTACT, Optional Card C. 
RWFORC  Wall forces. 
SBTOUT 
Seat belt output file 
SECFORC  Cross section forces.  See *DATABASE_CROSS_SECTION_OPTION. 
SLEOUT 
Sliding interface energy.  See *CONTROL_ENERGY 
SPCFORC 
SPC reaction forces. 
SPHOUT 
SPH data.  See *DATABASE_HISTORY_OPTION. 
SSSTAT 
Subsystem data.  See *DATABASE_EXTENT_SSSTAT. 
SWFORC  Nodal constraint reaction forces (spot welds and rivets). 
TPRINT 
Thermal  output  from  a  coupled  structural/thermal  or  thermal  only 
analysis. 
  Includes  all  nodes  unless  *DATABASE_HISTORY_-
NODE_OPTION is also provided in the keyword input. 
TRHIST 
Tracer particle history information.  See *DATABASE_TRACER. 
OPTION2, if it set, must be set to FILTER, and this can only be used when OPTION1 is 
set to NCFORC.  When set to FILTER the keyword requires an additional data card, see 
Card 2 below.  
To  include  global  and  subsystem  mass  and  inertial  properties  in  the  glstat  and  ssstat 
files  add  the  keyword  option  MASS_PROPERTIES  as  show  below.    If  this  option  is 
active the current mass and inertia properties are output including the principle inertias 
and  their  axes.    Mass  of  deleted  nodes  and  rigid  bodies  are  not  included  in  the 
calculated properties.
GLSTAT_MASS_PROPERTIES 
SSSTAT_MASS_PROPERTIES 
This  is  an  option  for  the  glstat  file  to  include 
mass and inertial properties. 
This  is  an  option  for  the  ssstat  file  to  include 
mass and inertial properties for the subsystems. 
  Card 1 
Variable 
1 
DT 
2 
3 
4 
5 
6 
7 
8 
BINARY 
LCUR 
IOOPT 
OPTION1  OPTION2  OPTION3  OPTION4 
Type 
F 
I 
I 
I 
F/I 
Default 
0. 
1 or 2 
none 
0. 
0 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DT 
DESCRIPTION
Time  interval  between  outputs.    If  DT  is  zero,  no  output  is
printed. 
BINARY 
Flag  for  binary  output.    See  remarks  under  "Output  Files  and
Post-Processing" in Appendix O, “LS-DYNA MPP User Guide.” 
EQ.1: ASCII file is written: 
This  is  the  default  for  shared 
memory parallel (SMP) LS-DYNA executables. 
EQ.2: Data  written  to  a  binary  database  “binout”,  which 
contains  data  that  would  otherwise  be  output  to  the
ASCII file.  The ASCII file in this case is not created.  This
is the default for MPP LS-DYNA executables. 
EQ.3: ASCII  file  is  written  and  the  data  is  also  written  to  the
binary database (NOTE: MPP LS-DYNA executables will 
only produce the binary database). 
Optional curve ID specifying time interval between dumps.  Use
*DEFINE_CURVE  to  define  the  curve;  abscissa  is  time  and
ordinate is time interval between dumps. 
Flag to govern behavior of the plot frequency load curve defined
by LCUR: 
EQ.1: At the time each plot is generated, the load curve value is
added  to  the  current  time  to  determine  the  next  plot
time.(this is the default behavior) 
EQ.2: At the time each plot is generated, the next plot time, 𝑡, is 
LCUR 
IOOPT
VARIABLE   
DESCRIPTION
computed so that 
𝑡 = the current time + LCUR(𝑡) . 
EQ.3:  A  plot  is  generated  for  each  abscissa  point  in  the  load
curve  definition.    The  actual  value  of  the  load  curve  is
ignored. 
OPTION1 applies to either the bndout, nodout or elout files.  For 
the  nodout  file  OPTION1  is  a  real  variable  that  defines  the  time 
interval between outputs for the high frequency file, nodouthf.  If 
OPTION1 is zero, no output is printed.  Nodal points that are to
be  output  at  a  higher  frequency  are  flagged  using  HFO  in  the 
DATABASE_HISTORY_NODE_LOCAL input. 
For  the  elout  file  OPTION1  is  an  integer  variable  that  gives  the 
number  of  additional  history  variables  written  into  the  elout  file 
for  each  integration  point  in  the  solid  elements.    See  Remark  7
below for the elout file and Remark 9 for the bndout file. 
OPTION2  applies  to  either  the  bndout,  nodouthf  or  elout  files. 
For  the  nodouthf  OPTION2  defines  the  binary  file  flag  for  the
high frequency nodouthf file.  See BINARY above. 
For  the  elout  file  OPTION2  is  an  integer  variable  that  gives  the 
number  of  additional  history  variables  written  into  the  elout  file 
for  each  integration  point  in  the  shell  elements.    See  Remark  7
below for the elout file and Remark 9 for the bndout file. 
OPTION3 applies to the bndout and elout files only.  For the elout
file  OPTION3  is  an  integer  variable  that  gives  the  number  of 
additional  history  variables  written  into  the  elout  file  for  each 
integration point in the thick shell elements.  See Remark 7 below 
for the elout file and Remark 9 for the bndout file. 
OPTION4 applies to the bndout and elout files only.  For the elout
file  OPTION4  is  an  integer  variable  that  gives  the  number  of 
additional  history  variables  written  into  the  elout  file  for  each 
integration point in the beam elements.  See Remark 7 below for 
the elout file and Remark 9 for the bndout file. 
OPTION1 
OPTION2 
OPTION3 
OPTION4
The following Card 2 applies only to *DATABASE_NCFORC_FILTER 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RATE 
CUTOFF  WINDOW
TYPE 
Type 
F 
F 
F 
Default 
none 
none 
none 
I 
0 
0 
0 
0 
0 
  VARIABLE   
DESCRIPTION
RATE 
Time interval 𝑇 between filter sampling. 
CUTOFF 
Frequency cut-off 𝐶 in Hz. 
WINDOW 
The width of the window 𝑊 in units of time for storing the single, 
forward 
  filtering  required  for  the  TYPE = 2  filter  option. 
Increasing  the  width  of  the  window  will  increase  the  memory
required  for  the  analysis.    A  window  that  is  too  narrow  will
reduce  the  amplitude  of  the  filtered  result  significantly,  and
values below 15 are not recommended for that reason.  In general,
the  results  for  the  TYPE = 2  option  are  sensitive  to  the  width  of 
the window and experimentation is required. 
TYPE 
Flag for filtering options.   
EQ.0: No filtering (default). 
EQ.1: Single pass, forward Butterworth filtering. 
EQ.2: Two  pass  filtering  over  the  specified  time  window.
Backward Butterworth filtering is applied to the forward
Butterworth  results  that  have  been  stored.    This  option
improves the phase accuracy significantly at the expense
of memory. 
The file names and corresponding unit numbers are: 
Description 
I/O Unit # File Name 
Airbag statistics 
43 
Automatic tiebreak damage  92 
ASCII database 
Boundary conditions 
44 
46 
abstat 
atdout 
avsflt 
bndout (nodal forces and energies)
Description 
I/O Unit # File Name 
Smug animator database 
Discrete elements 
40 
36 
Discrete elements mass flow 219 
Discrete beam elements 
215 
Element data 
Contact entities 
Global data 
Joint forces 
Material energies 
MOVIE file family 
MPGS file family 
Nastran/BDF file 
Nodal interface forces 
Nodal force group 
Nodal point data 
Pulley element data 
Pressure tube data 
Rigid body data 
Resultant interface forces 
Rigidwall forces 
Seat belts 
Cross-section forces 
Interface energies 
SPC reaction forces 
SPH element data 
Subsystems statistics 
Nodal constraint resultants 
Thermal output 
Tracer particles 
34 
48 
35 
53 
37 
50 
50 
49 
38 
45 
33 
216 
421 
47 
39 
32 
52 
31 
51 
41 
68 
58 
42 
73 
70 
defgeo 
deforc 
demflow 
disbout 
elout 
gceout 
glstat 
jntforc 
matsum 
moviennn.xxx where.nnn=001-999 
mpgsnnn.xxx where nnn = 001-999
nasbdf  
ncforc 
nodfor 
nodout 
pllyout 
prtube 
rbdout 
rcforc 
rwforc 
sbtout 
secforc 
sleout 
spcforc 
sphout 
ssstat 
swforc (spot welds/rivets) 
tprint 
trhist
Output Components for ASCII Files. 
ABSTAT 
BNDOUT 
DCFAIL 
  x, y, z force 
  energies 
  moment (rigid bodies) 
volume 
pressure 
internal energy 
input mass flow rate 
output mass flow rate 
mass 
temperature 
density 
failure function 
normal term 
bending term 
shear term 
weld area 
effective strain rate 
axial force 
shear force 
torsional moment 
bending moment 
DEFORC 
x, y, z force 
ELOUT 
(t)Shells 
xx, yy, zz stress 
xy, yz, zx stress 
plastic strain 
xx, yy, zz strain† 
xy, yz, zx strain† 
Beams 
axial force resultant 
s shear resultant 
t shear resultant 
s moment resultant 
t moment resultant 
torsional resultant 
Solids 
xx, yy, zz stress 
xy, yz, zx stress 
effective stress 
yield function 
xx, yy, zz strain† 
xy, yz, zx strain† 
†  Strains written for solids and for lower and upper integration points of shells 
and tshells if STRFLG = 1 in *DATABASE_EXTENT_BINARY. 
GCEOUT 
x, y, z force 
x, y, z moment
time step 
kinetic energy 
internal energy 
sprint and damper energy 
hourglass energy 
system damping energy 
sliding interface energy 
eroded kinetic energy 
eroded internal energy 
eroded hourglass energy 
added mass  
GLSTAT 
total energy 
external work 
total and initial energy 
energy ratio without eroded energy 
element & part ID controlling time step 
global x, y, z velocity 
time per zone cycle 
joint internal energy 
stonewall energy 
rigid body stopper energy 
percentage [mass] increase 
JNTFORC 
x, y, z force 
x, y, z moment 
MATSUM 
kinetic energy 
internal energy 
hourglass energy 
x, y, z momentum 
x, y, z rigid body velocity 
eroded internal energy 
eroded kinetic energy 
added mass 
NCFORC 
NODOUT 
X force 
Y force 
Z force 
  x, y, z displacement 
  X, y, z velocity 
  X, y, z acceleration 
  X, y, z rotation 
  X, y, z rotational velocity 
  X, y, z rotation acceleration 
NODFOR 
X, y.  z force 
PRTUBE 
cross section area 
pressure 
velocity 
density
PLLYOUT 
RBDOUT 
RCFORC 
adjacent beam IDs 
slip 
slip rate 
resultant force 
wrap angle 
  x, y, z displacement 
  x, y, z velocity 
  x, y, z acceleration 
x, y, z force 
Mass of nodes in contact 
RWFORC 
SECFORC 
SLEOUT 
normal 
x, y, z force 
x, y, z force 
x, y, z moment 
x, y, z center 
area 
resultant force 
slave energy 
master energy 
frictional energy 
SPCFORC 
SWFORC 
SPHOUT 
x, y, z force 
x, y, z moment 
  axial force 
  shear force 
failure function 
  weld length 
resultant moment 
torsion 
xx, yy, zz stress 
xy, yz, zx stress 
density 
number of neighbors 
xx, yy, zz strain 
xy, yz, zx strain 
half of smoothing length 
plastic strain 
particle active state 
effective stress 
temperature 
xx,yy,zz strain rate 
xy,yz,zx strain rate 
SPH to SPH coupling 
forces 
Remarks: 
1.  Discrepancies Between “matsum” and “glstat” Output.  The kinetic energy 
quantities in the matsum and glstat files may differ slightly in values for several 
reasons.    First,  the  energy  associated  with  added  mass  (from  mass-scaling)  is 
included in the glstat calculation, but is not included in matsum.  Secondly, the 
energies are computed element by element in matsum for the deformable mate-
rials  and,  consequently,  nodes  which  are  merged  with  rigid  bodies  will  also 
have their kinetic energy included in the rigid body total.  Furthermore, kinetic 
energy is computed from nodal velocities in glstat and from element midpoint 
velocities in matsum. 
2.  PRINT  Keyword  Option  on  *PART.    The  PRINT  option  in  the  part  definition 
allows some control over the extent of the data that is written into the matsum 
and  rbdout  files.    If  the  print  option  is  used  the  variable  PRBF  can  be  defined 
such that the following numbers take on the meanings: 
EQ.0:  default is taken from the keyword *CONTROL_OUTPUT, 
EQ.1:  write data into rbdout file only, 
EQ.2:  write data into matsum file only, 
EQ.3:  do not write data into rbdout and matsum. 
Also see CONTROL_OUTPUT and PART_PRINT. 
3.  The  Restart  Feature.    This  keyword  is  also  used  in  the  restart  phase,  see 
*RESTART.  Thus, the output interval can be changed when restarting. 
4.  LS-PrePost.  All information in the files except in AVSFLT, MOVIE, and MPGS 
can  also  be  plotted  using  LS-PrePost.    Arbitrary  cross  plotting  of  results  be-
tween ASCII files is easily handled. 
5.  The “rcforc” File.  Resultant contact forces reported in rcforc are averaged over 
the preceding output interval. 
6.  Spring and Damper Energy.  “Spring and damper energy” reported in glstat 
is  a  subset  of  “Internal  energy”.      The  “Spring  and  damper  energy”  includes 
internal energy of discrete elements, seatbelt elements, and that associated with 
joint stiffness.   
7.  OPTIONn  Field  for  “elout”.    OPTION1,  OPTION2,  OPTION3,  and  OPTION4 
give the number of additional history variables output for the integrated solids, 
shells,  thick  shells,  and  beams,  respectively.    Within  this  special  option,  each 
integration point is printed with its corresponding history data.  No integration 
points are averaged.  This is different than the default output where the stress 
data within a shell ply of a fully integrated shell, for example, are averaged and 
then  written  as  output.    The  primary  purpose  of  this  database  extension  is  to 
allow  the  actual  integration  point  stress  data  and  history  variable  data  to  be 
checked.  There are no transformations applied to either the output stresses or 
history data.
8.  The Failure Function.  The failure function reported to the DCFAIL database is 
set to zero when the weld fails.  If damage is active, then it is set to the negative 
of the damage scale factor which goes from 1 to 0 as damage grows. 
9.  OPTIONn  Field  for  “bndout”.    For  the  bndout  file,  OPTION1  controls  the 
nodal  force  group  output,  OPTION2  controls  the  concentrated  force  output, 
OPTION3  controls  the  pressure  boundary  condition  output,  and  OPTION4 
controls the velocity/displacement/acceleration nodal boundary conditions.  If 
the value is 0 or left blank, the category is included (the default), and if it is 1, 
the category is not included in the bndout file.  
10.  Contents of “glstat”.  The glstat table above includes all items that may appear 
in the glstat data.  The items that are actually written depend on the contents of 
the  input  deck.      For  example,  hourglass  energy  appears  only  if  HGEN = 2  in 
*CONTROL_ENERGY  and  added  mass  only  appears  if  DT2MS < 0  in  *CON-
TROL_TIMESTEP. 
11.  Element  ID  Controlling  the  Time  Step.    The  element  ID  controlling  the  time 
step is included in the glstat data but is not read by LS-PrePost.   If the element 
ID  is  of  interest  to  the  user,  the  ASCII  version  of  the  glstat  file  can  be  opened 
with a text editor. 
12.  The  FILTER  Option.    The  FILTER  option  uses  a  Butterworth  filter  for  the 
forward,  single  pass  filtering  and  the  backward,  double  pass  filtering  options.  
The  forward  filtered  output  𝑌(𝑛)  at  sampling  interval  𝑛  is  obtained  from  the 
solution value 𝑋(𝑛) using the formula 
𝑌(𝑛) = 𝑎0𝑋(𝑛) + 𝑎1𝑋(𝑛 − 1) + 𝑎2𝑋(𝑛 − 2) + 𝑏1𝑌(𝑛 − 1) + 𝑏2𝑌(𝑛 − 2) 
where the coefficients are 
𝜔𝑑 = 2𝜋 (
0.6
) 1.25 
𝜔𝑎 = tan(𝜔𝑎 𝑇/2) 
2/(1 + √2𝜔𝑎 + 𝜔𝑎
2) 
𝑎0 = 𝜔𝑎
𝑎1 = 2𝑎0 
𝑎2 = 𝑎0 
𝑏1 = 2(1 − 𝜔𝑎
2)/(1 + √2𝜔𝑎 + 𝜔𝑎
2) 
𝑏2 = (−1 + √2𝜔𝑎 − 𝜔𝑎
2)/(1 + √2𝜔𝑎 + 𝜔𝑎
2) 
The  two  previous  solution  values  and  filtered  values  at  𝑛 − 1  and  𝑛 − 2  are 
stored.
Backward  filtering  improves  the  phase  response  of  the  filtered  output.    It  is 
performed according to the formula 
𝑍(𝑛) = 𝑎0𝑌(𝑛) + 𝑎1𝑌(𝑛 + 1) + 𝑎2𝑌(𝑛 + 2) + 𝑏1𝑍(𝑛 + 1) + 𝑏2𝑍(𝑛 + 2) 
where 𝑍(𝑛) is the backward filtered value at sample time 𝑛.  This implies that 
all  the  forward  filtered  values  𝑌(𝑛)  are  stored  during  the  analysis,  and  that 
would  require  a  prohibitive  amount  of  memory.    To  limit  the  amount  of 
memory required, the forward filtered values at stored for the time interval 𝑊, 
where the number of stored states is 𝑊/𝑇, and the backward filtering is applied 
starting at the last saved value of the forward filtered values.  As the window 
width increases, the filtered values approach the values that would be obtained 
from storing all of the forward filtered values.  
The  results  of  the  backward  filtering  are  sensitive  to  the  window  width,  and 
experimentation  with  the  width  is  necessary  to  obtain  good  results  with  the 
minimum window width.  A window width of at least 10 to 15 times the sam-
ple rate 𝑇 should be used as a starting point.  Some applications may require a 
window  width  that  is  much  larger.    The  required  window  width  decreases  as 
the  cut-off  frequency  increases.    Or,  to  put  it  another  way,  the  window  width 
must be increased to make the filtered output smoother.  
As an example, a random series of numbers between 0 and 1 was generated and 
filtered  at  intervals  of  0.1  milliseconds  with  cut-off  frequencies  from  60  Hz  to 
420 Hz.  The reverse filtering was applied with various window widths to de-
termine how many forward filtered states must be saved to achieve fixed levels 
of accuracy compared to complete reverse filtering from the last state to the first 
state.  The results are shown in the table below.  Note that the error is calculated 
only for the first state and the numbers being filtered are random. This example 
should only be used as a very rough guide that indicates the overall trends and not as a 
recommendation for specific problems. 
Cut-off 
Frequency 
No.  of States 
50% Error 
No.  of States 
25% Error 
No.  of States 
10% Error 
No.  of States 
5% Error 
No.  of States 
1% Error 
60 Hz 
120 Hz 
180 Hz 
240 Hz 
300 Hz 
360 Hz 
420 Hz 
26 
13 
8 
6 
5 
5 
4 
33 
16 
10 
8 
6 
6 
5 
55 
30 
22 
17 
12 
10 
9 
68 
37 
26 
19 
15 
12 
10 
87 
44 
30 
23 
18 
16 
15
*DATABASE 
Purpose:    For  each  ALE  group  (or  material),  this  card  controls  the  output  for  element 
time-history variables (in a tabular format that can be plotted in LS-PrePost by using the 
XYPlot button). 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DTOUT 
SETID 
Type 
F 
I 
Default 
none 
none 
Variable  Cards.    Optional  cards  that  can  be  used  to  add  more  variables  with  the 
volume fractions in the database (the volume fractions are always output).  Include as 
many cards as necessary.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VAR 
VAR 
VAR 
VAR 
VAR 
VAR 
VAR 
VAR 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
DTOUT 
Time interval between the outputs 
SETID 
ALE element set ID. 
If  the  model  is  1D  (*SECTION_ALE1D),  the  set  should  be
*SET_BEAM 
If  the  model  is  2D  (*SECTION_ALE2D),  the  set  should  be
*SET_SHELL 
If  the  model  is  3D  (*SECTION_SOLID),  the  set  should  be
*SET_SOLID
VARIABLE   
DESCRIPTION
VAR 
Variable rank in the following list: 
EQ.1:  xx-stress 
EQ.2:  yy-stress 
EQ.3:  zz-stress 
EQ.4:  xy-stress 
EQ.5:  yz-stress 
EQ.6:  zx-stress 
EQ.7:  plastic strain 
EQ.8: 
internal energy 
EQ.9:  bulk viscosity 
EQ.10:  previous volume 
EQ.11:  pressure 
EQ.12:  mass 
EQ.13:  volume 
EQ.14:  density 
EQ.15:  kinetic energy 
If  there  is  a  blank  column  between  2  variable  ranks,  the  list
between  these  2  ranks  is  selected.    For  example,  if  the  card  is  as
follows: 
1, ,6 
The 6 stresses are added to the database.  
Remarks: 
1.  The .xy  files  are  created  when  the  termination  time  is  reached  or  if  one  of  the 
following  switches  (after  pressing  the  keys  Ctrl  -  C)  stops  the  job:  sw1,  stop, 
quit.  During the run, they can be created with the switch sw2. 
2.  The  .xy  files  are  created  by  element.    There  is  a  curve  by  ALE  group  (or 
material).  A last curve can be added for volume averaged variables.
*DATABASE 
Purpose:  For each ALE group (or material), this card activates extra output for: 
1.  material volume: alematvol.xy, 
2.  material mass: alematmas.xy, 
3. 
internal energy: alematEint.xy, 
4.  kinetic energy: alematEkin.xy, 
5. 
and kinetic energy loss during the advection: alematEkinlos.xy. 
These files are written in the “.xy” format, which LS-PrePost can plot with its “XYPlot” 
button. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DTOUT 
BOXLOW 
BOXUP 
Type 
F 
Default 
none 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
DTOUT 
Time interval between the outputs 
BOXLOW, BOXUP 
Range of *DEFINE_BOX ids.  BOXLOW is the lower bound
for the range while BOXUP is the upper bound.  The series
of volumes covered by the specified range of *DEFINE_BOX
determines  the  mesh  regions  for  which  ALE  material  data
are to be output. 
Remarks: 
The “.xy” files are created at termination or if one of the following switches (Ctrl-C) is 
encountered: sw2, sw1, stop, quit.
*DATABASE_BINARY_OPTION1_OPTION2 
keyword 
This 
*DATABASE_EXTENT_BINARY. 
used 
is 
to 
request 
binary 
output. 
See 
also 
Choices for OPTION1 are: 
BLSTFOR 
Blast pressure database.  See also *LOAD_BLAST_ENHANCED and 
Remark 3. 
CPMFOR 
Corpuscular Particle Method interface force database.  see Remark 2. 
D3DRLF 
Dynamic relaxation database. 
D3DUMP 
D3PART 
D3PLOT 
D3PROP 
D3THDT 
Database for restarts.  Define output frequency in cycles. 
Database  for  subset  of  parts.    See  also  *DATABASE_EXTENT_BI-
NARY and *DATABASE_EXTENT_D3PART. 
Database  for  entire  model.    See  also  *DATABASE_EXTENT_BINA-
RY. 
Database  containing  property  data.    See  *DATABASE_BINARY_-
D3PROP. 
Database  containing  time  histories  for  subsets  of  elements  and 
nodes.  See *DATABASE_HISTORY.  This database includes no ge-
ometry. 
DEMFOR 
DEM interface force database.  See Remark 5. 
FSIFOR 
FSILNK 
RUNRSF 
INTFOR 
ALE interface force database.  See Remark 1. 
ALE interface linking database.  See Remark 4. 
Database for restarts.  Define output frequency in cycles. 
Contact interface database.  Its file name must either be given using 
the  FILE  option  or  on  the  execution  line  using  "S=".    Also  see 
*CONTACT variables SPR and MPR. 
PBMFOR 
Particle Blast Method interface force database.   
D3CRACK 
Option to control output interval for ASCII “aea_crack” file for the 
Winfrith  concrete  model  (*MAT_084/085).    Oddly,  this  command 
does not control the output of the binary crack database for the Win-
frith  concrete  model.    The  binary  crack  database  is  written  when 
“q=”  appears  on  the  execution  line  and  its  output  interval  is  taken 
from *DATABASE_BINARY_D3PLOT,  It is used by LS-PrePost to-
gether with the D3PLOT database to display cracks in the deformed 
Winfrith concrete materials.
OPTION2  only  applies  when  OPTION1  is  set  to  INTFOR  and  the  only  choice  for 
OPTION2  is  FILE.    *DATABASE_BINARY_INTFOR_FILE  requires  one  extra  line  of 
input that specifies the name of the intfor database. 
The D3DUMP and the RUNRSF options create complete databases which are necessary 
for  restarts,  see  *RESTART.    When  RUNRSF  is  specified,  the  same  file  is  overwritten 
after each interval, an option allows a series of files to be overwritten in a cyclic order.  
When  D3DUMP  is  specified,  a  new  restart  file  is  created  after  each  interva,  thus  a 
“family” of files is created numbered sequentially, e.g., d3dump01, d3dump02, etc.  The 
default  file  names  are  runrsf  and  d3dump  unless  other  names  are  specified  on  the 
execution line, see the INTRODUCTION, EXECUTION SYNTAX.  Since all data held in 
memory is written into the restart files, these files can be quite large and care should be 
taken with the d3dump files not to create too many.  If *DATABASE_BINARY_D3PLOT 
is not specified in the keyword deck then the output interval for d3plot is automatically 
set to 1/20th the termination time. 
The  d3plot,  d3part,  d3drlf,  and  intfor  databases  contain  histories  of  geometry  and  of 
state variables.  Thus using these databases, one can, e.g., animate deformed geometry 
and plot time histories of element stresses and nodal displacements with LS-PrePost. 
The  d3thdt  database  contains  no  geometry  but  rather  time  history  data  for  element 
subsets  as  well  as  global  information,  see  *DATABASE_HISTORY.    This  data  can  be 
plotted with LS-PrePost.  The intfor database does not have a default filename and one 
must be specified by adding s=filename to the execution line. 
Similarly, for the fsifor database, a unique filename must be specified on the execution 
line  with  h=filename;  see  the  INTRODUCTION,  EXECUTION  SYNTAX.    The  file 
structure is such that each file contains the full geometry at the beginning, followed by 
the analysis generated output data at the specified time intervals. 
For the contents of the d3plot, d3part and d3thdt databases, see also the *DATABASE_-
EXTENT_BINARY  definition.    It  is  possible  to  restrict  the  information  that  is  dumped 
and consequently reduce the size of the databases.  The contents of the d3thdt database 
are also specified with the *DATABASE_HISTORY definition.  It should also be noted 
in  particular  that  the  databases  can  be  considerably  reduced  for  models  with  rigid 
bodies containing many elements. 
FILE Card: Provide this card only for *DATABASE_BINARY_INTFOR_FILE.
FILE Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
  VARIABLE   
FNAME 
FNAME 
A80 
none 
DESCRIPTION
Name  of  the  database  for  the  intfor  data.    S = filename  on  the 
execution line will override FNAME. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  DT/CYCL  LCDT/NR 
BEAM 
NPLTC 
PSETID 
CID 
Type 
Default 
F 
- 
I 
- 
I 
- 
I 
- 
I 
- 
I 
- 
D3PLOT Card.  Additional Card for D3PLOT option. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IOOPT 
RATE 
CUTOFF  WINDOW 
TYPE 
PSET 
Type 
Default 
I 
0 
F 
F 
F 
none 
none 
none 
I 
0 
I
VARIABLE   
DT / CYL 
NR 
LCDT 
DESCRIPTION
This field defines the time interval between output states, DT, for 
all options except D3DUMP, RUNRSF, and D3DRLF. 
For  D3DUMP,  RUNRSF,  and  D3DRLF  options  the  first  field
contains CYCL instead of DT.  These databases are updated every
CYCL convergence checks during the explicit dynamic relaxation
phase. 
Number  of  RUNning  ReStart  Files,  runrsf,  written  in  a  cyclical 
fashion.    The  default  is  1,  i.e.,  only  one  runrsf  file  is  created  and
the data therein is overwritten each time data is output. 
Optional load curve ID specifying time interval between dumps. 
This  variable  is  only  available  for  options  D3PLOT,  D3PART,
D3THDT, INTFOR and BLSTFOR.
VARIABLE   
BEAM 
NPLTC 
CID 
DESCRIPTION
Discrete  element  option  flag  (*DATABASE_BINARY_D3PLOT 
only). 
EQ.0: Discrete  spring  and  damper  elements  are  added  to  the
d3plot  database  where  they  are  displayed  as  beam  ele-
ments.  The discrete elements’ global 𝑥, global 𝑦, global 𝑧
and  resultant  forces  (moments),  and  change  in  length 
(rotation)  are  written  to  the  database  where  LS-PrePost 
(incorrectly)  labels  them  as  though  they  were  beam 
quantities,  i.e.,  axial  force,  S-shear  resultant,  T-shear  re-
sultant, etc. 
EQ.1: No  discrete  spring,  damper  and  seatbelt  elements  are
added to the d3plot database.  This option is useful when 
translating  old  LS-DYNA  input  decks  to  KEYWORD 
input.  In older input decks there is no requirement that
beam  and  spring  elements  have  unique  ID's,  and  beam
elements  may  be  created  for  the  spring  and  dampers
with  identical  ID's  to  existing  beam  elements  causing  a
fatal error.  However, this option comes with some limi-
tations and, therefore, should be used with caution. 
1.  Contact  interfaces  which  are  based  on  part  IDs
of seatbelt elements will not be properly gener-
ated if this option is used. 
2.  DEFORMABLE_TO_RIGID will not work if PID 
refers to discrete, damper, or seatbelt elements.
EQ.2: Discrete  spring  and  damper  elements  are  added  to  the
d3plot  database  where  they  are  displayed  as  beam  ele-
ments  (similar  to  option  0).    In  this  option  the  element
resultant  force  is  written  to  its  first  database  position
allowing beam axial forces and spring resultant forces to
be  plotted  at  the  same  time.    This  can  be  useful  during 
some post-processing applications. 
This  flag,  set  in  *DATABASE_BINARY_D3PLOT,  also  affects  the 
display  of  discrete  elements  in  several  other  databases  such  as
d3drlf, d3part. 
DT = ENDTIME/NPLTC.    Applies  to  D3PLOT  and  D3PART
options only.  This overrides the DT specified in the first field. 
Coordinate system ID for FSIFOR and FSILNK, see *DEFINE_CO-
ORDINATE_SYSTEM.
VARIABLE   
PSETID 
DESCRIPTION
Part  set  ID  for  D3PART  and  D3PLOT  options  only.    See  *SET_-
PART.    Parts  in  PSETID  will  excluded  in  the  d3plot  database. 
Onlyparts in PSETID are included in the d3part database. 
IOOPT 
This variable applies to the D3PLOT option only.  Flag to govern
behavior of the plot frequency load curve defined by LCDT: 
EQ.1: At the time each plot is generated, the load curve value is
added to the current time to determine the next plot time
(this is the default behavior). 
EQ.2: At the time each plot is generated, the next plot time T is
computed  so  that  T = the  current  time  plus  the  load 
curve value at time T. 
EQ.3: A  plot  is  generated  for  each  abscissa  point  in  the  load
curve  definition.    The  actual  value  of  the  load  curve  is
ignored. 
RATE 
Time interval 𝑇 between filter sampling. 
CUTOFF 
Frequency cut-off 𝐶 in Hz. 
WINDOW 
The width of the window 𝑊 in units of time for storing the single, 
forward  filtering  required  for  the  TYPE = 2  filter  option. 
Increasing  the  width  of  the  window  will  increase  the  memory
required  for  the  analysis.    A  window  that  is  too  narrow  will
reduce  the  amplitude  of  the  filtered  result  significantly,  and
values below 15 are not recommended for that reason.  In general,
the  results  for  the  TYPE = 2  option  are  sensitive  to  the  width  of 
the window and experimentation is required. 
TYPE 
Flag for filtering options.   
EQ.0: No filtering (default). 
EQ.1: Single pass, forward Butterworth filtering. 
EQ.2: Two  pass  filtering  over  the  specified  time  window.
Backward Butterworth filtering is applied to the forward
Butterworth  results  that  have  been  stored.    This  option 
improves the phase accuracy significantly at the expense
of memory.
PSET 
*DATABASE_BINARY 
DESCRIPTION
Part  set  ID  for  filtering.    If  no  set  is  specified,  all  parts  are
included.  For each element integration point in the d3plot file, 24 
words  of  memory  are  required  in  LS-DYNA  for  the  single  pass 
filtering, and more for the two pass filtering.  Specifying PSET is
recommended to minimize the memory requirements. 
Remarks: 
1.  FSIFOR.    *DATABASE_BINARY_FSIFOR  only  applies  to  models  having 
penalty-based coupling between Lagrangian and ALE materials (CTYPE=4 or 5 
in  the  coupling  card,  *CONSTRAINED_LAGRANGE_IN_SOLID).    When 
*DATABASE_FSI  is  defined,  a  few  pieces  of  coupling  information  of  some 
Lagrangian surface entities interacting with the ALE materials may be output as 
history  parameters  into  a  file  called  “dbfsi”.    Coupling  pressure  is  one  of  the 
output variables.  However, this coupling pressure is averaged over the whole 
surface entity being monitored.  To obtain coupling pressure contour plot as a 
function of time over the coupled surface, a user can define the  *DATABASE_-
BINARY_FSIFOR keyword.  To use it, three things must be done: 
a)  The INTFORC parameter (*CONSTRAINED_LAGRANGE_IN_SOLID, 4th 
row, 3rd column) must be turned ON (INTFORC = 1).   
b)  A  *DATABASE_BINARY_FSIFOR  card  is  defined  controlling  the  output 
interval.    The  time  interval  between  output  is  defined  by  the  parameter 
DT in this card. 
c)  This interface force file is activated by executing LS-DYNA as follows:  
lsdyna i=inputfilename.k ...  h=interfaceforcefilename 
LS-DYNA will then write out the segment coupling pressure and forces 
to a binary interface force file for contour plotting over the whole simula-
tion interval. 
To plot the binary data in this file, type: lsprepost interfaceforcefilename. 
For  example,  when  all  3  of  the  above  actions  are  taken,  and  assuming 
“h” is set to “fsifor”, then a series of “fsifor##” binary files are output for 
contour plotting.  To plot this, type “lsprepost fsifor” (without the dou-
ble quotes).
2.  CPMFOR. 
  *DATABASE_BINARY_CPMFOR  applies 
to  models  using 
*AIRBAG_PARTICLE feature which controls the output interval of CPM inter-
face force file.  This interface force file is activated by executing LS-DYNA with 
command line option (cpm=). 
lsdyna i=inputfilename.k … cpm=interfaceforce_filename 
CPM  interface  force  file  stores  segment’s  coupling  pressure  and  forces.    The 
coupling pressure is averaged over each segment without considering the effect 
of ambient pressure, 𝑃atm. 
3.  BLSTFOR.    The  BLSTFOR  database  is  not  available  for  two  dimensional 
axisymmetric analysis. 
4.  FSILNK.    The  *DATABASE_BINARY_FSILNK  variant  writes  the  selected 
*CONSTRAINED_LAGRANGE_IN_SOLID  interface’s  segment  pressure  to the 
fsilink file for the next analysis without ALE meshes. 
lsdyna i=inputfilename.k … fsilink=filename 
5.  DEMFOR.    *DATABASE_BINARY_DEMFOR  applies  to  models  using  DEM 
coupling  option  *DEFINE_DE_TO_SURFACE_COUPLING.    This  card  will 
control the output interval of DEM interface force file. This interface force file is 
activated by LS-DYNA command line option (dem=). 
lsdyna  i=inputfilename.k … dem=interfaceforce_filename 
DEM interface force file stores segment’s coupling pressure and forces. 
6.  PBMFOR.  *DATABASE_BINARY_PBMFOR applies to models using *PARTI-
CLE_BLAST  feature  which  controls  the  output  interval  of  PBM  interface  force 
file.  This interface force file is activated by executing LS-DYNA with command 
line option (pbm=). 
lsdyna  i=inputfilename.k … pbm=interfaceforce_filename 
PBM interface force file stores segment’s coupling pressure and forces.
*DATABASE_BINARY 
Purpose:    This  card  causes  LS-DYNA  to  add  the  part,  material,  equation  of  state, 
section,  and  hourglass  data  to  the  first  d3plot  file  or  else  write  the  data  to  a  separate 
database d3prop.  Rigidwall data can also be included.    LS-PrePost does not read the 
additional data so use of this command is of dubious benefit. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IFILE 
IMATL 
IWALL 
Type 
Default 
I 
1 
I 
0 
I 
0 
  VARIABLE   
IFILE 
DESCRIPTION
Specify  file  for  d3prop  output.    (This  can  also  be  defined  on  the
command  line  by  adding  d3prop = 1  or  d3prop = 2  which  also 
sets IMATL =  IWALL = 1) 
EQ.1: Output data at the end of the first d3plot file. 
EQ.2: Output data to the file d3prop. 
IMATL 
Output *EOS, *HOURGLASS, *MAT, *PART and *SECTION data.
EQ.0: No 
EQ.1: Yes 
IWALL 
Output *RIGIDWALL data. 
EQ.0: No 
EQ.1: Yes 
.
*DATABASE 
Purpose:    This  card  activates  an  ASCII  file  “cpm_sensor”.    Its  input  defines  sensors’ 
locations  based  on  the  positions  of  some  Lagrangian  segments.    The  output  gives  the 
history  of  the  velocity,  temperature,  density  and  pressure  averaged  on  the  number  of 
particles contained in the sensors.  This card is activated only when the *AIRBAG_PAR-
TICLE card is used. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DT 
BINARY 
Type 
F 
I 
Sensor Definition Cards.  Each card defines one sensor.  This card may be repeated to 
define multiple sensors.  Input stops when the next “*” Keyword is found.  
6 
7 
8 
  Card 2 
1 
2 
3 
4 
Variable 
SEGID 
OFFSET 
R/LX 
LEN/LY 
Type 
I 
F 
F 
F 
5 
LZ 
F 
  VARIABLE   
DESCRIPTION
DT 
Output interval 
BINARY 
Flag for the binary file 
EQ.1:  ASCII file is written,  
EQ.2:  Data written to the binary file “binout”, 
EQ.3:  ASCII  file  is  written  and  the  data  written  to  the  binary
file “binout”. 
SEGID 
Segment set ID 
OFFSET 
Offset  distance  between  the  center  of  the  sphere  sensor  and  the
segment center.  If it is positive, Or, the distance between the base
of  the  cylinder  and  the  segment  center  while  LENGTH  is  not
zero.    it  is  on  the  side  pointed  to  by  the  segment  normal  vector. 
See remarks1 and 3.
R/LX 
*DATABASE_CPM_SENSOR 
DESCRIPTION
Radius(sphere)/length  in  local  X  direction(rectangular)  of  the
sensor.  See remarks 2 and 3.   
LEN/LY 
Length(cylinder)/length  in  local  Y  direction(rectangular)  of  the
sensor. 
LZ 
Length in local Z direction(rectangular) of the sensor see remark 4
Remarks: 
1.  Each segment  has a sensor.  The distance  between the segment center and the 
sensor center is defined by OFFSET (2nd parameter on the 2nd line) in the normal 
direction  defined  by  the  segment.    This  distance  is  constant:  the  sensor  moves 
along with the segment.  
2.  The sensor is a sphere with a radius given by RADIUS (3rd parameter on the 2nd 
line).  
3.  OFFSET should be larger than RADIUS to prevent the segment from cutting the 
sphere.  For cylindrical sensor, OFFSET is the distance from segment to the base 
of the cylinder.  
4.  For  rectangular  sensor,  OFFSET  is  the  distance  from  reference  segment  to  the 
sensor.  The sensor is defined using the segment’s coordinates system.  The base 
point is n1 and local X direction is along the vector n2 - n1.  The local Z direc-
tion  is  the  segment  normal  direction  and  local  Y  direction  is  constructed  by 
local X and Z directions.  
5.  The output parameters in the “cpm_sensor” file are:  
velx 
vely 
velz 
velr 
temp 
dens 
pres 
 =   x-velocity 
 =   y-velocity 
 =   z-velocity 
 =   velocity 
 =  
 =   density 
 =   pressure 
temperature 
These  values  are  averaged  on  the  number  of  particles  in  the  sensor.    RADIUS 
should  be  large  enough  to  contain  a  reasonable  number  of  particles  for  the 
averages. 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|. 
$ INPUT: 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|. 
*DATABASE_CPM_SENSOR
0.01 
$   SEGSID    OFFSET    RADIUS    LENGTH 
       123       5.0       5.0    
       124      -0.2       0.1    
       125       0.7       0.6       1.0 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|.. 
$ The segment set id: 123 has 1 segment. 
$ The segment set id: 123 has 1 segment. 
$ The segment set id: 123 has 11 segments. 
$ Each segment has an ID defined in D3HSP 
$ The D3HSP file looks like the following: 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|.. 
Segments for sensor          1 
  Sensor id        n1        n2        n3        n4 
         1      3842      3843      3848      3847 
 Segments for sensor          2 
  Sensor id        n1        n2        n3        n4 
         2      3947      3948      3953      3952 
 Segments for sensor          3 
  Sensor id        n1        n2        n3        n4 
         3      3867      3868      2146      2145 
         4      3862      3863      3868      3867 
         5      3857      3858      3863      3862 
         6      3852      3853      3858      3857 
         7      3847      3848      3853      3852 
         8      3837      3838      3843      3842 
         9      3842      3843      3848      3847 
        10      3832      3833      3838      3837 
        11      3827      3828      3833      3832 
        12      3822      3823      3828      3827 
        13      1125      1126      3823      3822 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|..
*DATABASE_CROSS_SECTION_OPTION1_{OPTION2} 
Option 1 includes: 
PLANE 
SET 
To define an ID and heading for the database cross section use the option: 
ID 
Purpose:  Define a cross section for resultant forces written to ASCII file secforc. 
1.  For  the  PLANE  option,  a  set  of  two  cards  is  required  for  each  cross  section.  
Then a cutting plane has to be defined, see Figure 14-1. 
2. 
If the SET option is used, just one card is needed which identifies a node set and 
at  least  one  element  set.    In  this  case  the  node  set(s)  defines  the  cross  section, 
and  the  forces  from  the  elements  belonging  to  the  element  set(s)  are  summed 
up  to  calculate  the  section  forces.    Thus  the  element  set(s)  should  include  ele-
ments on only one side (not both sides) of the cross section. 
The  cross-section  should  cut  through  deformable  elements  only,  not  rigid  bodies.  
Cutting through master segments for deformable solid element spot welds can lead to 
incorrect section forces since the constraint forces are not accounted for in the force and 
moment  summations.    Beam  element  modeling  of  welds  do  not  require  any  special 
precautions. 
ID Card.  Additional card for ID keyword option. 
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CSID 
Type 
I 
HEADING 
A70 
The  heading  is  picked  up  by  some  of  the  peripheral  LS-DYNA  codes  to  aid  in  post-
processing. 
  VARIABLE   
DESCRIPTION
CSID 
Cross section ID.  This must be a unique number. 
HEADING 
Cross section descriptor.  It is suggested that unique descriptions
be used.
Plane Card 1.  First additional card for PLANE keyword option. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PSID 
XCT 
YCT 
ZCT 
XCH 
YCH 
ZCH 
RADIUS 
Type 
Default 
I 
0 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
Plane Card 2.  Second additional card for PLANE keyword option. 
  Card 2 
1 
2 
3 
4 
5 
Variable 
XHEV 
YHEV 
ZHEV 
LENL 
LENM 
Type 
F 
Default 
0. 
F 
0. 
F 
F 
F 
0. 
infinity 
infinity 
global 
6 
ID 
I 
7 
8 
ITYPE 
I 
0 
The set option requires that the equivalent of the automatically generated input by the 
cutting  plane  capability  be  identified  manually  and  defined  in  sets.    All  nodes  in  the 
cross-section  and  their  related  elements  that  contribute  to  the  cross-sectional  force 
resultants must be defined. 
Set Card.  Additional Card for the SET keyword option. 
  Card 1 
1 
2 
3 
4 
5 
6 
Variable 
NSID 
HSID 
BSID 
SSID 
TSID 
DSID 
Type 
I 
I 
Default 
required 
0 
I 
0 
I 
0 
I 
0 
I 
0 
7 
ID 
I 
global 
8 
ITYPE 
I
*DATABASE_CROSS_SECTION 
Resultants are computed
on this plane
Origin of cutting plane
Figure  14-1.    Definition  of  cutting  plane  for  automatic  definition  of  interface
for cross-sectional forces.  The automatic definition does not check for springs
and  dampers in the section.   For  best results the  cutting  plane should cleanly
pass  through  the  middle  of  the  elements,  distributing  them  equally  on  either
side.  Elements that intersect the edges of the cutting plane are deleted from the
the cross-section. 
  VARIABLE   
DESCRIPTION
CSID 
PSID 
XCT 
YCT 
ZCT 
XCH 
Optional ID for cross  section.  If not specified cross  section ID is 
taken to be the cross section order in the input deck. 
Part set ID.  If zero all parts are included. 
𝑥-coordinate  of  tail  of  any  outward  drawn  normal  vector,  N, 
originating  on  wall  (tail)  and  terminating  in  space  (head),  see 
Figure 14-1. 
𝑦-coordinate of tail of normal vector, 𝐍. 
𝑧-coordinate of tail of normal vector, 𝐍. 
𝑥-coordinate of head of normal vector, 𝐍.
VARIABLE   
DESCRIPTION
YCH 
ZCH 
RADIUS 
𝑦-coordinate of head of normal vector, 𝐍. 
𝑧-coordinate of head of normal vector, 𝐍. 
Optional  radius.    If  a  radius  is  set  (radius ≠  0),  then  circular  cut 
plane centered at (XCT, YCT ,ZCT) of radius = RADIUS, with the 
normal  vector  originating  at  (XCT,  YCT,  ZCT)  and  pointing 
towards  (XCH,  YCH,  ZCH)  will  be  created.    In  this  case  the
variables  XHEV,  YHEV,  ZHEV,  LENL,  and  LENM,  which  are
defined on the 2nd card will be ignored. 
XHEV 
YHEV 
ZHEV 
LENL 
𝑥-coordinate of head of edge vector, 𝐋. 
𝑦-coordinate of head of edge vector, 𝐋. 
𝑧-coordinate of head of edge vector, 𝐋. 
Length of edge 𝑎, in 𝐋 direction. 
LENM 
Length of edge 𝑏, in 𝐌 direction. 
NSID 
HSID 
BSID 
SSID 
TSID 
DSID 
ID 
Nodal set ID, see *SET_NODE_OPTION. 
Solid element set ID, see *SET_SOLID. 
Beam element set ID, see *SET_BEAM. 
Shell element set ID, see *SET_SHELL_OPTION. 
Thick shell element set ID, see *SET_TSHELL. 
Discrete element set ID, see *SET_DISCRETE. 
Rigid  body  ,  accelerometer  ID  ,  or  coordinate  ID, 
see  *DEFINE_COORDINATE_NODES.    The  force  resultants  are 
output  in  the  updated  local  system  of  the  rigid  body  or 
accelerometer.    For  ITYPE = 2,  the  force  resultants  are  output  in 
the updated local coordinate system if FLAG = 1 in *DEFINE_CO-
ORDINATE_NODES or if NID is nonzero in *DEFINE_COORDI-
NATE_VECTOR.
ITYPE 
*DATABASE_CROSS_SECTION 
DESCRIPTION
Flag that specifies whether ID above pertains to a rigid body, an
accelerometer, or a coordinate system. 
EQ.0: rigid body, 
EQ.1: accelerometer, 
EQ.2: coordinate system.
Available options include: 
*DATABASE 
AVS 
BINARY 
D3PART 
INTFOR 
MOVIE 
MPGS 
SSSTAT 
Purpose:  Control to some extent the content of specific output databases.   
The  BINARY  option  of  *DATABASE_EXTENT  applies  to  the  binary  databases  d3plot, 
d3thdt, and d3part.  In the case of the d3part database, variables set using the D3PART 
option  will  override  the  corresponding  variables  of  the  BINARY  option.    See  also 
*DATABASE_BINARY_OPTION. 
The  AVS,  MOVIE,  and  MPGS  databases  will  be  familiar  to  users  that  have  a  use  for 
those databases.
*DATABASE_EXTENT_AVS 
This  command  controls  content  written  to  the  avsflt  database.    See  AVSFLT  option  to 
*DATABASE card. 
Varriable Cards.  Define as many cards as  needed.  Input ends at next keyword (“*”) 
card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VTYPE 
COMP 
Type 
I 
I 
  VARIABLE   
DESCRIPTION
VTYPE 
Variable type: 
EQ.0:  node, 
EQ.1:  brick, 
EQ.2:  beam, 
EQ.3:  shell, 
EQ.4:  thick shell. 
Component 
components from the following tables can be chosen: 
the  corresponding  VTYPE, 
  For 
ID. 
integer
VTYPE.EQ.0:  Table 10.1, 
VTYPE.EQ.1:  Table 10.2, 
VTYPE.EQ.2:  not supported, 
VTYPE.EQ.3:  Table 10.3, 
VTYPE.EQ.4:  not supported. 
COMP 
Remarks: 
The  AVS  database  consists  of  a  title  card,  then  a  control  card  defining  the  number  of 
nodes,  brick-like  elements,  beam  elements,  shell  elements,  and  the  number  of  nodal 
vectors,  NV,  written  for  each  output  interval.    The  next  NV  lines  consist  of  character 
strings  that  describe  the  nodal  vectors.    Nodal  coordinates  and  element  connectivity 
follow.    For  each  state  the  solution  time  is  written,  followed  by  the  data  requested
below.  The last word in the file is the number of states.  We recommend creating this 
file and examining its contents, since the organization is relatively transparent. 
Table 14-2.  Nodal Quantities 
Component ID 
Quantity  
1 
2 
3 
x, y, z-displacements 
x, y, z-velocities 
x, y, z-accelerations 
Table 14-3.  Brick Element Quantities 
Component ID 
1 
2 
3 
4 
5 
6 
7 
Quantity 
x-stress 
y-stress 
z-stress 
xy-stress 
yz-stress 
zx-stress 
effective plastic strain
Table 14-4.  Shell and Thick Shell Element Quantities 
Component ID 
Quantity 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
11 
12 
13 
14 
15 
16 
17 
18 
19 
20 
21 
22 
23 
24 
25 
26 
27 
28 
29 
midsurface x-stress 
midsurface y-stress 
midsurface z-stress 
midsurface xy-stress 
midsurface yz-stress 
midsurface xz-stress 
midsurface effective plastic strain 
inner surface x-stress 
inner surface y-stress 
inner surface z-stress 
inner surface xy-stress 
inner surface yz-stress 
inner surface zx-stress 
inner surface effective plastic strain 
outer surface x-stress 
outer surface y-stress 
outer surface z-stress 
outer surface xy-stress 
outer surface yz-stress 
outer surface zx-stress 
outer surface effective plastic strain 
bending moment-mxx (4-node shell) 
bending moment-myy (4-node shell) 
bending moment-mxy (4-node shell) 
shear resultant-qxx (4-node shell) 
shear resultant-qyy (4-node shell) 
normal resultant-nxx (4-node shell) 
normal resultant-nxx (4-node shell) 
normal resultant-nxx (4-node shell)
Component ID 
Quantity 
30 
31 
32 
33 
34 
35 
36 
37 
38 
39 
40 
41 
42 
43 
44 
45 
46 
47 
48 
49 
50 
51 
52 
53 
54 
55 
56 
57 
58 
59 
thickness (4-node shell) 
element dependent variable 
element dependent variable 
inner surface x-strain 
inner surface y-strain 
inner surface z-strain 
inner surface xy-strain 
inner surface yz-strain 
inner surface zx-strain 
outer surface x-strain 
outer surface y-strain 
outer surface z-strain 
outer surface xy-strain 
outer surface yz-strain 
outer surface zx-strain 
internal energy 
midsurface effective stress 
inner surface effective stress 
outer surface effective stress 
midsurface max.  principal strain 
through thickness strain 
midsurface min.  principal strain 
lower surface effective strain 
lower surface max.  principal strain 
through thickness strain 
lower surface min.  principal strain 
lower surface effective strain 
upper surface max.  principal strain 
through thickness strain 
upper surface min.  principal strain
Component ID 
Quantity 
60 
upper surface effective strain 
Table 14-5.  Beam Element Quantities 
Component ID 
Quantity 
1 
2 
3 
4 
5 
6 
x-force resultant 
y-force resultant 
z-force resultant 
x-moment resultant 
y-moment resultant 
z-moment resultant
*DATABASE_EXTENT_BINARY_{OPTION} 
Purpose:  Control to some extent the content of binary output databases d3plot, d3thdt, 
and  d3part.    See  also  *DATABASE_BINARY_OPTION  and  *DATBASE_EXTENT_D3-
PART.  The content of the binary output database intfor may be modified using *DATA-
BASE_EXTENT_INTFOR.  The option COMP  controls to the content of binary output 
databases d3plot and d3eigv.  When the option COMP is used, it will suppress most of 
settings in *DATABASE_EXTENT_BINARY. 
Available options include: 
<BLANK> 
COMP 
If no option is specified, use the following cards: 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NEIPH 
NEIPS 
MAXINT 
STRFLG 
SIGFLG 
EPSFLG 
RLTFLG 
ENGFLG 
Type 
Default 
I 
0 
I 
0 
Remarks 
  Card 2 
1 
2 
I 
3 
1 
3 
I 
1 
I 
1 
I 
1 
I 
1 
I 
0 
10 
4 
5 
6 
7 
8 
Variable 
CMPFLG 
IEVERP 
BEAMIP 
DCOMP 
SHGE 
STSSZ 
N3THDT 
IALEMAT 
Type 
Default 
I 
0 
I 
0 
Remarks 
I 
0 
2 
I 
1 
I 
1 
I 
1 
I 
2 
I
*DATABASE_EXTENT_BINARY 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  NINTSLD  PKP_SEN 
SCLP 
HYDRO 
MSSCL 
THERM 
INTOUT  NODOUT 
Type 
Default 
I 
1 
I 
0 
F 
1.0 
I 
0 
I 
0 
I 
0 
A 
A 
none 
none 
Remarks 
  Card 4 
1 
2 
3 
4 
5 
6 
4 
7 
4 
8 
Variable 
DTDT 
RESPLT 
NEIPB 
Type 
Default 
I 
1 
I 
0 
I 
0 
For COMP option, use Card 1 below (no Cards 2-4) 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IGLB 
IXYZ 
IVEL 
IACC 
ISTRS 
ISTRA 
ISED 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
Remarks
VARIABLE   
NEIPH 
NEIPS 
DESCRIPTION
Number of additional integration point history variables written to
the binary databases (d3plot, d3part, d3drlf) for solid elements and 
SPH  particles.    The  integration  point  data  is  written  in  the  same
order that it is stored in memory-each material model has its own 
history  variables  that  are  stored.    For  user  defined  materials  it  is
important  to  store  the  history  data  that  is  needed  for  plotting 
before the data which is not of interest.  See also *DEFINE_MATE-
RIAL_HISTORIES.    For  output  of  additional  integration  point
history  variables  for  solid  elements  to  the  elout  database,  see  the 
variable OPTION1 in *DATABASE_ELOUT. 
Number of additional integration point history variables written to
the  binary  databases  (d3plot,  d3part,  d3drlf)  for  both  shell  and 
thick  shell  elements  for  each  integration  point,  see  NEIPH  above
and *DEFINE_MATERIAL_HISTORIES.  For output of additional 
integration  point  history  variables  for  shell  and  thick  shell
elements  to  the  elout  database,  see  the  variables  OPTION2  and 
OPTION3, respectively, in *DATABASE_ELOUT.
VARIABLE   
MAXINT 
DESCRIPTION
Number  of  shell  and  thick  shell  through-thickness  integration 
points for which output is written to d3plot.  This does not apply 
to strain tensor output flagged by STRFLG. 
MAXINT 
(def = 3) 
number of 
Integration 
Points 
Description 
> 3 
(even & odd)
results  are  output  for  the  outermost 
(top) 
(bottom) 
and 
integration  points 
together  with 
results for the neutral axis. 
innermost 
1 
All three results are identical. 
3 
3 
 > 3 
≤ MAXINT 
≠ 3 
Even 
< 0 
Any 
for 
the 
Results 
first  MAXINT 
integration points in the element will 
be output. 
See  above.    This  will  exclude  mid-
results,  whereas  when 
surface 
MAXINT = 3 mid-surface results are 
calculated and reported. 
integration  points  are 
MAXINT 
output  for  each  in  plane  integration 
point  location  and  no  averaging  is 
used.    This  can  greatly  increase  the 
size  of  the  binary  databases  d3plot, 
d3thdt, and d3part. 
See Remark 1 for more information.
VARIABLE   
DESCRIPTION
STRFLG 
STRFLG is interpreted digit-wise STRFLG = [𝑁𝑀𝐿], 
STRFLG = 𝐿 + 𝑀 × 10 + 𝑁 × 100 
L.EQ.1:  Write strain tensor data to d3plot and elout.  For shell 
and thick shell elements two tensors are written, one at
the  innermost  and  one  at  the  outermost  integration
point.  For solid elements a single strain tensor is writ-
ten. 
M.EQ.1:  Write plastic strain data to d3plot. 
N.EQ.1:  Write thermal strain data to d3plot. 
Examples.  For STRFLG = 11 (011) LS-DYNA will write both strain 
and plastic strain tensors, but no thermal strain tensors.  Whereas
for STRFLG = 110, LS-DYNA will write plastic and thermal strain 
tensors but no strain tensors.  For more information and supported
elements and materials, see Remark 10. 
SIGFLG 
Flag for including the stress tensor for shells and solids. 
EQ.1: include (default), 
EQ.2: exclude for shells, include for solids. 
EQ.3: exclude for shells and solids. 
EPSFLG 
Flag for including the effective plastic strains for shells and solids.
EQ.1: include (default), 
EQ.2: exclude for shells, include for solids. 
EQ.3: exclude for shells and solids. 
RLTFLG 
Flag for including stress resultants in the shell LS-DYNA database:
EQ.1: include (default), 
EQ.2: exclude. 
ENGFLG 
Flag for including shell internal energy density and shell thickness.
EQ.1: include (default), 
EQ.2: exclude.
CMPFLG 
*DATABASE_EXTENT_BINARY 
DESCRIPTION
Flag  to  indicate  the  coordinate  system  for  output  of  stress  and
strain in solids, shells and thick shells comprised of orthotropic or
anisotropic materials.  See Remark 4. 
EQ.-1:  Same as 1, but for *MAT_FABRIC (forms 14 and -14) and 
*MAT_FABRIC_MAP the stress and strain is in engineer-
ing quantities instead of Green-Lagrange strain and 2nd 
Piola-Kirchhoff stress. 
EQ.0:  global  coordinate  system  with  exception  of  elout  for 
shells . 
EQ.1:  local  material  coordinate  system  (as  defined  by  AOPT
and associated parameters in the *MAT input, and if ap-
plicable,  by  angles  B1,  B2,  etc.    in  *SECTION_SHELL, 
*SECTION_TSHELL,  or  *PART_COMPOSITE,  and  by 
optional  input  in  the  *ELEMENT  data).    CMPFLG = 1 
affects both d3plot and elout databases. 
IEVERP 
Every output state for the d3plot database is written to a separate 
file. 
EQ.0: more than one state can be on each plot file, 
EQ.1: one state only on each plot file. 
BEAMIP 
Number  of  beam  integration  points  for  output.    This  option  does
not apply to beams that use a resultant formulation.  See Remark 
2.
VARIABLE   
DESCRIPTION
DCOMP 
Data compression to eliminate rigid body data: 
EQ.1: off (default), no rigid body data compression, 
EQ.2: on, rigid body data compression active, 
EQ.3: off,  no  rigid  body  data  compression,  but  all  nodal
velocities and accelerations are eliminated from the data-
base. 
EQ.4: on,  rigid  body  data  compression  active  and  all  nodal
velocities and accelerations are eliminated from the data-
base. 
EQ.5: on,  rigid  body  data  compression  active  and  rigid  nodal
data are eliminated from the database.  Only 6 DOF rigid
body motion is written. 
EQ.6: on, rigid body data compression active, rigid nodal data,
and  all  nodal  velocities  and  accelerations  are  eliminated
from the database.  Only 6 DOF rigid body motion is writ-
ten. 
SHGE 
Flag for including shell hourglass energy density. 
EQ.1: off (default), no hourglass energy written, 
EQ.2: on. 
STSSZ 
Flag for including shell element time step, mass, or added mass. 
EQ.1: off (default), 
EQ.2: output time step size, 
EQ.3: output mass, added mass, or time step size. 
See Remark 3 below. 
N3THDT 
Flag for including material energy in d3thdt database. 
EQ.1: off, energy is NOT written to d3thdt database, 
EQ.2: on (default), energy is written to d3thdt database. 
IALEMAT 
Output solid part ID list containing ALE materials. 
EQ.1: on (default)
NINTSLD 
PKP_SEN 
SCLP 
HYDRO 
*DATABASE_EXTENT_BINARY 
DESCRIPTION
Number  of  solid  element  integration  points  written  to  the  LS-
DYNA  database.    When  NINTSLD  is  set  to  1  (default)  or  to  any
value other than 8, integration point values are averaged and only
those averages are written output.  To obtain values for individual
integration points, set NINTSLD to 8, even if the multi-integration 
point solid has fewer than 8 integration points. 
Flag to output the peak pressure and surface energy computed by
each contact interface into the interface force database.   To obtain
the  surface  energy,  FRCENG,  must  be  sent  to  1  on  the  control
contact  card.    When  PKP_SEN = 1,  it  is  possible  to  identify  the 
energies generated on the upper and lower shell surfaces, which is
important  in  metal  forming  applications.    This  data  is  mapped
after each H-adaptive remeshing. 
EQ.0: No data is written 
EQ.1: Output the peak pressures and surface energy by contact
interface 
A scaling parameter used in the computation of the peak pressure.
This parameter is generally set to unity (the default), but it must be
greater than 0. 
Either 3, 5 or 7 additional history variables useful to shock physics
are output as the last history variables to d3plot (does not apply to 
elout).  For HYDRO = 1, the internal energy per reference volume, 
the  reference  volume,  and  the  pressure  from  bulk  viscosity  are
added  to  the  database,  and  for  HYDRO = 2,  the  relative  volume 
and current density are also added.  For HYDRO = 4, two further 
variables are added: volumetric strain (defined as relative volume
– 1.0), and Hourglass energy per unit initial volume. 
MSSCL 
Output  nodal  information  related  to  mass  scaling  into  the  d3plot
database.  This option can be activated if and only if DT2MS < 0.0, 
see control card *CONTROL_TIMESTEP. 
EQ.0: No data is written 
EQ.1: Output incremental nodal mass 
EQ.2: Output percentage increase in nodal mass 
See Remark 3.
VARIABLE   
THERM 
DESCRIPTION
Output  of  thermal  data  to  d3plot.    The  use  of  this  option 
(THERM > 0)  may  make  the  database  incompatible  with  other  3rd
party software. 
EQ.0: (default) output temperature 
EQ.1: output temperature 
EQ.2: output temperature and flux 
EQ.3: output  temperature,  flux,  and  shell  bottom  and  top
surface temperature 
INTOUT 
Output  stress/strain  at  all  integration  points  for  detailed  element
output  in  the  ASCII  file  eloutdet.    DT  and  BINARY  of  *DATA-
BASE_ELOUT apply to eloutdet.  See Remark 4. 
EQ.STRESS: when stress output is required 
EQ.STRAIN:  when strain output is required 
EQ.ALL: 
when both stress and strain output are required 
NODOUT 
Output  extrapolated  stress/strain  at  connectivity  nodes  for
detailed element output in the ASCII file eloutdet.  DT and BINA-
RY of *DATABASE_ELOUT apply to eloutdet.  See Remark 4. 
EQ.STRESS: 
when stress output is required 
EQ.STRAIN: 
when strain output is required 
EQ.ALL: 
when  both  stress  and  strain  output  are 
required 
EQ.STRESS_GL:  when nodal averaged stress output along the 
global coordinate system is required 
EQ.STRAIN_GL:  when nodal averaged strain output along the 
global coordinate system is required 
EQ.ALL_GL: 
for  global  nodal  averaged  stress  and  strain 
output 
DTDT 
Output of node point Δtemperature/Δtime data to d3plot. 
EQ.0: (default) no output 
EQ.1: output Δ𝑇/Δ𝑡
RESPLT 
*DATABASE_EXTENT_BINARY 
DESCRIPTION
Output of translational and rotational residual forces to d3plot and 
d3iter. 
EQ.0: No output 
EQ.1: Output residual 
NEIPB 
Number  of  additional  element  or  integration  point  history
variables  written  to  the  binary  databases  (d3plot,  d3part,  d3drlf) 
for beam elements, see NEIPH above, BEAMIP and *DEFINE_MA-
TERIAL_HISTORIES. 
  For  output  of 
additional integration point history variables for beam elements to
the  elout  database,  see  the  variable  OPTION4  in  *DATABASE_-
ELOUT. 
  See  also  Remark 12. 
IGLB 
Output flag for global data 
EQ.0: no 
EQ.1: yes 
IXYZ 
Output flag for geometry data 
EQ.0: no 
EQ.1: yes 
IVEL 
Output flag for velocity data 
EQ.0: no 
EQ.1: yes 
IACC 
Output flag for acceleration data 
EQ.0: no 
EQ.1: yes 
ISTRS 
Output flag for stress data 
EQ.0: no 
EQ.1: yes 
ISTRA 
Output flag for strain data 
EQ.0: no 
EQ.1: yes 
ISED 
Output flag for strain energy density data 
EQ.0: no 
EQ.1: yes
Remarks: 
1.  MAXINT  Field.    If  MAXINT  is  set  to  3  then  mid-surface,  inner-surface  and 
outer-surface stresses are output at the center of the element.  For an even num-
ber of integration points, the points closest to the center are averaged to obtain 
the midsurface values.  If multiple integration points are used in the shell plane, 
the stresses at the center of the element are found by computing the average of 
these points.  For MAXINT equal to 3, LS-DYNA assumes that the data for the 
user defined integration rules are ordered from bottom to top even if this is not 
the case.  If MAXINT is not equal to 3, then the stresses at the center of the ele-
ment  are  output  in  the  order  that  they  are  stored  for  the  selected  integration 
rule.  If multiple points are used in plane the stresses are first averaged. 
2.  BEAMIP Field.  Beam stresses are output if and only if BEAMIP is greater than 
zero.  In this latter case the data that is output is written in the same order that 
the integration points are defined.  The data at each integration point consists of 
the  following  five  values  for  elastic-plastic  Hughes-Liu  beams:  the  normal 
stress, 𝜎𝑟𝑟; the transverse shear stresses, σrs and σtr; the effective plastic strain, 
and the axial strain which is logarithmic.  For beams that are not elastic-plastic, 
the first history variable, if any, is output instead of the plastic strain.  For the 
beam  elements  of  Belytschko  and  his  co-workers,  the  transverse  shear  stress 
components  are  not  used  in  the  formulation.    No  data  is  output  for  the  Be-
lytschko-Schwer resultant beam. 
3.  Mass Scaling.  If mass scaling is active, the output of the time step size reveals 
little  information  about  the  calculation.    If  global  mass  scaling  is  used  for  a 
constant  time  step,  the  total  element  mass  is  output;  however,  if  the  mass  is 
increased so that a minimum time step size is maintained (DT2MS is negative), 
the added mass is output.  Also, see the control card *CONTROL_TIMESTEP. 
4.  Output  Coordinate  System.    Output  coordinate  system  used.    When  the 
parameters: INTOUT or NODOUT is set to STRESS, STRAIN, or ALL, the out-
put coordinate system of the data, similar to the ASCII file elout,  is determined 
by CMPFLG  in *DATABASE_EXTENT_BINARY. 
a)  When NODOUT is set to STRESS, STRAIN , or ALL.  Each node of the el-
ement nodal connectivity will be output.  See Example 1. 
b)  Nodal  output  when    NODOUT  is  set  to  STRESS_GL,  STRAIN_GL,  or 
ALL_GL.  Averaged nodal results are calculated by summing up all con-
tributions from elements sharing the common node, and then dividing the 
total by the number of contributing elements.  Averaged nodal values are 
always output in the global coordinate system.  See Example 2. 
5.  Contents  of  eloutdet.    Available  stress/strain  components  in  eloutdet  stress 
components includes  6 stress  components (sig-𝑥𝑥, sig-𝑦𝑦, sig-𝑧𝑧, sig-𝑥𝑦, sig-𝑦𝑧,
sig-𝑧𝑥), yielding status, and effective plastic strain.  Strain components includes 
6 strain components 
6.  Shell Element Output at Integration Points.  stresses at all integration points 
can be output.  The strain at the top and bottom integration layer can be output.   
At  a  connective  node  the  extrapolated  stress  and  strain  at  the  top  and  bottom 
layer can be output 
7.  Thick Shells.  Thick shell element output includes the six stress components at 
each  integration  point.    Strain  at the  top  and  bottom  layer  can  be  output.      At 
the element node, values at the bottom layer are extrapolated to yield the values 
of  nodes  1-4,  and  values  at  the  top  layer  are  extrapolated  to  yield  values  of 
nodes 5-8.   
8. 
Integration  Point  Locations.    Stresses  and  strain  at  all  integration  points  can 
be output.  The integration point order is as follows: 
a)  point #1 is the point closest to node #1 in the connectivity array 
b)  point #2 is the closest point to node #2, etc 
c)  For tetrahedrons type 4, 16 and 17 with 5 integration points, point #5 is the 
midpoint. 
d)  For the nodal points, values at the integration points are extrapolated. 
9.  Reporting Residual Forces and Moments.  The output of residual forces and 
moments is supported for implicit and double precision only.  With this option 
the forces and moments appear under the Ndv button in the fringe menu in LS-
PrePost.  The residual for rigid bodies is distributed to the slave nodes for the 
body without scaling for the purpose of capturing the complete residual vector. 
10.  Calculation  of  Strains  (STRFLG).    The  strain  tensor  𝜺  that  are  output  to  the 
d3plot  database  are  calculated  using  proper  time  integration  of  the  rate-of-
deformation  tensor  𝐃.    More  specifically,  to  assert  objectivity  of  the  resulting 
strain, it is for solids using a Jaumann rate of strain whereas for shells it uses the 
co-rotational  strain  rate.    In  mathematical  terms  the  integration  is  using  the 
following strain rates 
𝛆̇ = 𝐃 − 𝛆𝐖 + 𝐖𝛆
(solids)
𝛆̇ = 𝐃 − 𝛆𝛀  + 𝛀𝛆
(shells)
where  𝐖  is  the  spin  tensor  and  𝛀 = 𝐐̇ 𝐐T  is  the  rotational  velocity  of  the  co-
rotational system 𝐐 used for the shell element in question, taking into account 
invariant  node  numbering  and  such.    This  is  to  say  that  the  resulting  strains 
would  be  equal  to  the  Cauchy  stress  for  a  hypo-elastic  material  (MAT_ELAS-
TIC)  with  a  Young’s  modulus  of  1  and  a  Poisson’s  ratio  of  0.    This  should  be
kept  in  mind  when  interpreting  the  results  since  they  are  not  invariant  to 
changes in element formulations and possibly nodal connectivities. 
11.  Plastic and Thermal Strain (STRFLG).  The algorithm for writing plastic and 
thermal strains, which is also activated using STRFLG, is a modification of the 
algorithm used for mechanical strains . 
a)  For  solids  the  element  average  strain in the global  system  having 6  com-
ponents is written (local system if CMPFLG is set). 
b)  For shells both plastic and thermal strains have 6 components.  The ther-
mal  strain  is  written  as  a  single  tensor  as  in  the  solid  case.    The  plastic 
strain output consists of 3 plane-averaged tensors: one for the bottom, one 
for the middle, and one for the top.  For an even number of through thick-
ness integration points, the middle is taken to be the average of the two in-
tegration points closest to the mid surface.  Currently, only the following 
element/materials  combinations  are  supported  but  other  will  be  added 
upon request. 
Thermal strain tensors 
Plastic strain tensors 
Shells 
Solids  Materials 
Shells 
Solids 
Materials 
2, 16, 23 
1, 2 
Add 
thermal 
expansion,
255 
2, 16, 23 
1, 2 
24, 255 
12.  History  Variables  for  Beams  (NEIPB).  In  general,  NEIPB  follows  the  same 
conventions  as  NEIPH  and  NEIPS  do  for  solid  and  shell  elements  and  is  sup-
ported in LS-PrePost v4.3 or later.  Average, min and max values for each ele-
ment are output, including data for resultant elements.  If BEAMIP is nonzero, 
then element data is complemented with BEAMIP integration point values that 
can be examined individually.  Beam history data is post-processed similarly to 
that of solid and shell element history data. 
Example 1: 
Excerpt  from  eloutdet  file  for  a  shell  element  with  two  through-thickness  integration 
points  and  four  in-plane  integration  points,  with  INTOUT = STRESS  and  NO-
DOUT = STRESS: 
element  materl 
     ipt  stress  sig-xx   sig-yy   sig-zz   sig-xy   sig0yz   sig-zx   yield         location 
       1-      1 
   1- 10 elastic  4.41E-2  2.51E-1  0.00E+0  7.76E-8  0.00E+0  0.00E+0  0.00E+0  int.  point  1 
   1- 10 elastic  4.41E-2  2.51E-1  0.00E+0  7.76E-8  0.00E+0  0.00E+0  0.00E+0  int.  point  2 
   1- 10 elastic  4.41E-2  2.51E-1  0.00E+0  7.76E-8  0.00E+0  0.00E+0  0.00E+0  int.  point  3 
   1- 10 elastic  4.41E-2  2.51E-1  0.00E+0  7.76E-8  0.00E+0  0.00E+0  0.00E+0  int.  point  4 
   1- 10 elastic  4.41E-2  2.51E-1  0.00E+0  7.76E-8  0.00E+0  0.00E+0  0.00E+0  node       21
1- 10 elastic  4.41E-2  2.51E-1  0.00E+0  7.76E-8  0.00E+0  0.00E+0  0.00E+0  node       22 
   1- 10 elastic  4.41E-2  2.51E-1  0.00E+0  7.76E-8  0.00E+0  0.00E+0  0.00E+0  node       20 
   1- 10 elastic  4.41E-2  2.51E-1  0.00E+0  7.76E-8  0.00E+0  0.00E+0  0.00E+0  node       19 
   2- 10 elastic  4.41E-2  2.51E-1  0.00E+0  7.76E-8  0.00E+0  0.00E+0  0.00E+0  int.  point  1 
   2- 10 elastic  4.41E-2  2.51E-1  0.00E+0  7.76E-8  0.00E+0  0.00E+0  0.00E+0  int.  point  2 
   2- 10 elastic  4.41E-2  2.51E-1  0.00E+0  7.76E-8  0.00E+0  0.00E+0  0.00E+0  int.  point  3 
   2- 10 elastic  4.41E-2  2.51E-1  0.00E+0  7.76E-8  0.00E+0  0.00E+0  0.00E+0  int.  point  4 
   2- 10 elastic  4.41E-2  2.51E-1  0.00E+0  7.76E-8  0.00E+0  0.00E+0  0.00E+0  node       21 
   2- 10 elastic  4.41E-2  2.51E-1  0.00E+0  7.76E-8  0.00E+0  0.00E+0  0.00E+0  node       22 
   2- 10 elastic  4.41E-2  2.51E-1  0.00E+0  7.76E-8  0.00E+0  0.00E+0  0.00E+0  node       20 
   2- 10 elastic  4.41E-2  2.51E-1  0.00E+0  7.76E-8  0.00E+0  0.00E+0  0.00E+0  node       19 
Example 2: 
Excerpt from eloutdet file for averaged nodal strain: 
nodal strain calculations for time step   24  (at time 9.89479E+01 ) 
 node (global) 
          strain   eps-xx     eps-yy         eps-zz   eps-xy       eps-yz      eps-zx 
          1- 
 lower surface     2.0262E-01 -2.6058E-02 -7.5669E-02 -5.1945E-03  0.0000E+00  0.0000E+00 
 upper surface     2.0262E-01 -2.6058E-02 -7.5669E-02 -5.1945E-03  0.0000E+00  0.0000E+00 
          2- 
 lower surface     1.9347E-01  2.3728E-04 -8.3019E-02 -1.4484E-02  0.0000E+00  0.0000E+00 
 upper surface     1.9347E-01  2.3728E-04 -8.3019E-02 -1.4484E-02  0.0000E+00  0.0000E+00 
          3- 
 lower surface     2.0541E-01 -5.7521E-02 -6.3383E-02 -1.7668E-03  0.0000E+00  0.0000E+00 
 upper surface     2.0541E-01 -5.7521E-02 -6.3383E-02 -1.7668E-03  0.0000E+00  0.0000E+00 
       ⋮        ⋮       ⋮        ⋮       ⋮        ⋮        ⋮
*DATABASE 
The following cards control content to the d3part binary database (Card 3 is optional).  
The  parameters  given  here  will  supercede  the  corresponding  parameters  in  *DATA-
BASE_EXTENT_BINARY  when  writing  the  d3part  binary  database.    See  also  *DATA-
BASE_BINARY_D3PART  which  defines  the  output  interval  for  d3part  and  the  set  of 
part included in d3part.   
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NEIPH 
NEIPS 
MAXINT 
STRFLG 
SIGFLG 
EPSFLG 
RLTFLG 
ENGFLG 
Type 
Default 
I 
0 
I 
0 
Remarks 
  Card 2 
1 
2 
I 
3 
1 
3 
I 
0 
I 
1 
I 
1 
I 
1 
I 
1 
4 
5 
6 
7 
8 
Variable 
IEVERP 
SHGE 
STSSZ 
I 
0 
5 
I 
0 
6 
7 
8 
3 
4 
I 
0 
2 
Type 
Default 
  Card 3 
1 
Variable  NINTSLD 
Type 
Default 
I
NEIPH 
NEIPS 
MAXINT 
STRFLG 
*DATABASE_EXTENT_D3PART 
DESCRIPTION
Number  of  additional  integration  point  history  variables  written
to  the  binary  database  for  solid  elements.    The  integration  point
data is written in the same order that it is stored in memory-each 
material model has its own history variables that are stored.  For 
user defined materials it is important to store the history data that
is needed for plotting before the data which is not of interest. 
Number  of  additional  integration  point  history  variables  written
to the binary database for both shell and thick shell elements for 
each integration point, see NEIPH above. 
Number of shell integration points written to the binary database,
see also *INTEGRATION_SHELL.  If the default value of 3 is used 
then  results  are  output  for  the  outermost  (top)  and  innermost 
(bottom)  integration  points  together  with  results  for  the  neutral
axis.    If  MAXINT  is  set  to  3  and  the  element  has  1  integration
point then all three results will be the same.  If a value other than
3  is  used  then  results  for  the  first  MAXINT  integration  points  in 
the  element  will  be  output.    Note:    If  the  element  has  an  even
number  of  integration  points  and  MAXINT  is  not  set  to  3  then 
you  will  not  get  mid-surface  results.    See  Remarks  below.    If 
MAXINT is set to a negative number, MAXINT integration points 
are  output  for  each  in  plane  integration  point  location  and  no
averaging is used.   This can greatly increase the size of the binary
d3part database. 
Set  to  1  to  dump  strain  tensors  for  solid,  shell  and  thick  shell
elements  for  plotting  by  LS-PrePost  and  ASCII  file  elout.    For 
shell and thick shell elements two tensors are written, one at the
innermost  and  one  at  the  outermost  integration  point.    For  solid
elements a single strain tensor is written. 
SIGFLG 
Flag for including the stress tensor for shells. 
EQ.1: include (default), 
EQ.2: exclude. 
EPSFLG 
Flag for including the effective plastic strains for shells. 
EQ.1: include (default), 
EQ.2: exclude.
VARIABLE   
DESCRIPTION
RLTFLG 
Flag for including stress resultants for shells. 
EQ.1: include (default), 
EQ.2: exclude. 
ENGFLG 
Flag  for  including  shell  internal  energy  density  and  shell
thickness. 
EQ.1: include (default), 
EQ.2: exclude. 
IEVERP 
Every  plot  state  for  d3part  database  is  written  to  a  separate  file.
This option will limit the database to 1000 states: 
EQ.0: more than one state can be on each plot file, 
EQ.1: one state only on each plot file. 
SHGE 
Flag for including shell hourglass energy density. 
EQ.1: off (default), no hourglass energy written, 
EQ.2: on. 
STSSZ 
Flag for including shell element time step, mass, or added mass. 
EQ.1: off (default), 
EQ.2: output time step size, 
EQ.3: output mass, added mass, or time step size. 
See remark 3 below. 
NINTSLD 
Number of solid element integration points written.  The default
value is 1.  For solids with multiple integration points NINTSLD
may  be  set  to  8.    Currently,  no  other  values  for  NINTSLD  are
allowed.   For solids with multiple integration points, an average 
value is output if NINTSLD is set to 1.
*DATABASE_EXTENT_INTFOR 
The  following  card  controls  to  some  extent  the  content  of  the  optional  intfor  binary 
database.      See  also  *DATABASE_BINARY_INTFOR.    The  intfor  database  contains 
geometry and time history data pertaining to those contact surfaces which are flagged 
in  *CONTACT  with  the  variables  SPR  and/or MPR.      The  name  of  the intfor  database 
must be given on the execution line via “s=filename”. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NGLBV 
NVELO 
NPRESU  NSHEAR 
NFORC 
NGAPC 
NFAIL 
IEVERF 
Type 
Default 
I 
1 
I 
1 
I 
1 
I 
1 
I 
1 
I 
1 
I 
0 
I 
0 
Optional Card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NWEAR 
NWUSR 
NHUF 
Type 
Default 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
NGLBV 
Output global variables: 
EQ.-1:  no, 
EQ.1:  yes (default). 
NVELO 
Output nodal velocity: 
EQ.-1:  no, 
EQ.1:  yes (default).
VARIABLE   
DESCRIPTION
NPRESU 
Output pressures: 
EQ.-1:  no, 
EQ.1:  normal interface pressure (default), 
EQ.2:  normal interface pressure and peak pressure, 
EQ.3:  normal  interface  pressure,  peak  pressure  and  time  to
peak. 
NSHEAR 
Output shear stresses: 
EQ.-1:  no, 
EQ.1:  shear stress in r-direction and s-direction (default). 
NFORC 
Output forces: 
EQ.-1:  no, 
EQ.1:  𝑥-, 𝑦-, 𝑧-force at all nodes (default). 
NGAPC 
Output contact gaps at all nodes and surface energy density 
EQ.-1:  no, 
EQ.1:  yes (default). 
NFAIL 
Flag for display of deleted contact segments 
EQ.0:  all segments are displayed, 
EQ.1:  remove deleted contact segments from display. 
IEVERF 
Every interface force state for the “intfor” database is written to a 
separate file: 
EQ.0: more than one interface force state can  be on each intfor
file, 
EQ.1: one interface force output state only on each intfor file. 
NWEAR 
Output contact wear data, see *CONTACT_ADD_WEAR 
EQ.0: No output. 
GE.1: Output wear depth. 
GE.2: Output sliding distance. 
NWUSR 
Number  of  user  wear  history  variables  to  output  from  user
defined wear routines, see *CONTACT_ADD_WEAR.
Number  of  user  friction  history  variables  to  output  from  user
defined  friction  routines,  see  *USER_INTERFACE_FRICTION
(MPP only). 
*DATABASE 
  VARIABLE   
NHUF 
Remarks: 
For gaps in Mortar contact, see NGAPC, these are measured with respect to the nominal 
contact  surfaces  of  the  two  interacting  segments.    For  instance,  if  IGNORE = 2  on 
*CONTACT_...MORTAR  then  an  initial  penetration  𝑑  will  dislocate  the  slave  contact 
surface  in  the  negative  direction of  the  slave  surface  normal  𝒏.    The  gap 𝑔  reported to 
the  intfor  file  is  still  measured  between  the  master  and  slave  surface  neglecting  this 
dislocation, thus only physical gaps are reported. 
Wear outputs are governed by NWEAR and NWUSR, and requires the usage of a wear 
  For  NWEAR  the  “wear  depth” 
model  associated  with  the  contact  interface. 
(NWEAR.GE.1)  and  “sliding  distance”  (NWEAR.GE.2)  are  listed  under  the  Nodal 
fringe menu in LS-PrePost.  Following this, NWUSR user defined history variables are 
listed,  corresponding  to  user  wear  history variables  in  a  user  wear  routine.    These  are 
listed in the order that they are stored in the wear routine, see WTYPE.LT.0 on *CON-
TACT_ADD_WEAR.
*DATABASE 
This  keyword  controls  the  content  written  to  the  BYU  MOVIE  databases.    See  movie 
option on *DATABASE manual entry. 
Varriable Cards.  Define as many cards as  needed.  Input ends at next keyword (“*”) 
card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VTYPE 
COMP 
Type 
I 
I 
  VARIABLE   
DESCRIPTION
VTYPE 
Variable type: 
EQ.0: node, 
EQ.1: brick, 
EQ.2: beam, 
EQ.3: shell, 
EQ.4: thick shell. 
COMP 
.
Component 
components from the following tables can be chosen: 
the  corresponding  VTYPE, 
  For 
ID. 
integer
VTYPE.EQ.0:  Table 10.1 , 
VTYPE.EQ.1:  Table 10.2 , 
VTYPE.EQ.2:  not supported, 
VTYPE.EQ.3:  Table 10.3 , 
VTYPE.EQ.4:  not supported.
*DATABASE_EXTENT_MPGS 
Define as many cards as necessary.  The created MPGS databases consist of a geometry 
file and one file for each output database.  See MPGS option to *DATABASE keyword. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VTYPE 
COMP 
Type 
I 
I 
  VARIABLE   
DESCRIPTION
VTYPE 
Variable type: 
EQ.0: node, 
EQ.1: brick, 
EQ.2: beam, 
EQ.3: shell, 
EQ.4: thick shell. 
COMP 
Component 
components from the following tables can be chosen: 
the  corresponding  VTYPE, 
  For 
ID. 
integer
VTYPE.EQ.0:  Table 14-2 , 
VTYPE.EQ.1:  Table 14-3 , 
VTYPE.EQ.2:  not supported, 
VTYPE.EQ.3:  Table 14-4 , 
VTYPE.EQ.4:  not supported.
*DATABASE_EXTENT_SSSTAT_OPTION 
The only OPTION  is: 
ID 
The ID option allows the definition of a heading which will be written at the beginning 
of the ASCII file ssstat. 
Purpose:  This command defines one or more subsystems.  A subsystem is simply a set 
of  parts,  grouped  for  convenience.    The  ASCII  output  file  ssstat  provides  histories  of 
energy  (kinetic,  internal,  hourglass)  and  momentum  (x,  y,  and  z)  for  each  subsystem.   
The ssstat file is thus similar to glstat and matsum, but whereas glstat provides data for 
the  whole  model  and  matsum  provides  data  for  each  individual  part,  ssstat  provides 
data for each subsystem.  The output interval for the ssstat file is given using *DATA-
BASE_SSSTAT.  To also include histories of subsystem mass properties in the ssstat file, 
use *DATABASE_SSSTAT_MASS_PROPERTIES. 
For  *DATABASE_EXTENT_BINARY  without  the  ID  option,  the  following  card(s) 
apply.  Define as many cards as necessary.  Define one part set ID per subsystem, up to 
8 subsystems per card.   
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PSID1 
PSID2 
PSID3 
PSID4 
PSID5 
PSID6 
PSID7 
PSID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
For *DATABASE_EXTENT_BINARY_ID option, the following card(s) apply.  Define as 
many cards as necessary.  Define one part set ID per subsystem, 1 subsystem per card.   
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PSID1 
Type 
I 
HEADING1 
A70 
  VARIABLE   
DESCRIPTION
PSIDn 
Part set ID for subsystem n; see *SET_PART.
VARIABLE   
DESCRIPTION
HEADINGn 
Heading for subsystem n.
*DATABASE 
Purpose:  Process FATXML data.  FATXML is an open, standardized data format based 
on  the  Extensible  Markup  Language  (XML)  which  is  developed  by  the  German 
Research  Association  of  Automotive  Technology  (Forschungsvereinigung  Automobil-
technik  -  FAT).    It  is  designed  for  consistent  data  management  in  the  overall  CAE 
process chain.  A comprehensive explanation of the FATXML data format specification 
is given by Schulte-Frankenfeld and Deiters [2016].  
LS-DYNA reads all lines between this keyword and the next keyword recognized by the 
star  (*)  sign,  processes  the  data  with  respect  to  the  include  file  structure  and  writes 
everything together in one output file called ‘d3plot.xml’. 
Remarks: 
It  is  intended  that  a  corresponding  FE  model  consists  of  one  master  file  with  several 
associated  include  files  each  containing  a  description  by  *DATABASE_FATXML  data, 
usually  at  the  end  of  the  file.  The  master  file  loads  the  include  files  via  *INCLUDE_-
TRANSFORM  with  potential  offset  values  for  nodes,  elements,  parts,  etc.    (IDNOFF, 
IDEOFF, IDPOFF, …).  Finally, all data from different include files with different offsets 
are  collected  and  then  summarized  in  ‘d3plot.xml’.    Since  the  resulting  data  format  is 
public  domain,  Post-Processors  are  able  to  read  that  data  and  correlate  it  with  the 
associated CAE model. 
Example: 
... 
*DATABASE_FATXML 
<?xml version=”1.0”?> 
<CAE_META_DATA> 
  < PART_ID NAME=”TestCase”> 
    <PDM_DATA> 
      ... 
      <PDD_THICKNESS> 
        < THICKNESS ID=”123”>1.0</THICKNESS >  
        < THICKNESS ID=”124”>1.1</THICKNESS >  
        ...  
      </PDD_THICKNESS >  
      ... 
    </PDM_DATA >  
  </PART_ID >  
</CAE_META_DATA >  
*END
Purpose:  Define the output format for binary files. 
*DATABASE_FORMAT 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IFORM 
IBINARY 
Type 
Default 
Remarks 
I 
0 
1 
I 
0 
2 
  VARIABLE   
DESCRIPTION
IFORM 
Output format for d3plot and d3thdt files 
EQ.0: LS-DYNA database format (default), 
EQ.1: ANSYS database format, 
EQ.2: Both LS-DYNA and ANSYS database formats. 
IBINARY 
Word  size  of  the  binary  output  files  (d3plot,  d3thdt,  d3drlf  and 
interface files for 64 bit computer such as CRAY and NEC. 
EQ.0: default 64 bit format, 
EQ.1: 32 bit IEEE format 
Remarks: 
1.  The  ANSYS  output  option  is  not  available  in  MPP  and  is  not  universally 
available  in  SMP.    The  LS-DYNA  banner  in d3hsp  will  include  “ANSYS  data-
base format” under the list of “Features enabled” if the option is available. 
2.  By using this option one can reduce the size of the binary output files which are 
created by 64 bits computer such as CRAY and NEC.
*DATABASE_FREQUENCY_ASCII_OPTION 
Options for frequency domain ASCII databases with the default names given include: 
NODOUT_SSD  ASCII database for nodal results for SSD (displacement, velocity and 
acceleration).  See also *FREQUENCY_DOMAIN_SSD. 
  ELOUT_SSD 
ASCII  database  for  element  results  for  SSD  (stress  and  strain 
components).  See also *FREQUENCY_DOMAIN_SSD.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FMIN 
FMAX 
NFREQ 
FSPACE 
LCFREQ 
Type 
F 
F 
Default 
0.0 
0.0 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
FMIN 
FMAX 
Minimum frequency for output (cycles/time) 
Maximum frequency for output (cycles/time). 
NFREQ 
Number of frequencies for output. 
FSPACE 
Frequency spacing option for output: 
EQ.0:  linear 
EQ.1:  logarithmic 
EQ.2:  biased 
LCFREQ 
Load Curve ID defining the frequencies for output. 
Remarks: 
1.  The keyword defines output frequencies for NODOUT_SSD and ELOUT_SSD, 
and they can be different from output frequencies for D3SSD (which is defined 
by keyword *DATABASE_FREQUENCY_BINARY_D3SSD). 
2.  The ASCII databases NODOUT_SSD and ELOUT_SSD are saved in binout files.  
LS-PREPOST  is  able  to  read  the  binout  files  directly.    Users  can  also  convert 
these files to ASCII format simply feed them to the l2a program like this:
fmin
fmin
fmin
Linear Spacing
Logarithmic Spacing
fmax
fmax
mode n
mode n+1
mode n+2
Biased Spacing
fmax
Figure 14-6.  Spacing options of the frequency points. 
l2a  binout* 
3.  The  nodes 
to  be  output 
to  NODOUT_SSD  are  specified  by  card 
*DATABASE_HISTORY_NODE. 
4.  The solid, beam, shell and thick shell elements to be output to ELOUT_SSD are 
specified by the following cards: 
*DATABASE_HISTORY_SOLID_{OPTION} 
*DATABASE_HISTORY_BEAM_{OPTION} 
*DATABASE_HISTORY_SHELL_{OPTION} 
*DATABASE_HISTORY_TSHELL_{OPTION} 
5.  There are two methods to define the output frequencies. 
a)  The first method is to define FMIN, FMAX, NFREQ and FSPACE.  FMIN 
and  FMAX  specify  the  frequency  range  of  interest  and  NFREQ  specifies 
the  number  of  frequencies  at  which  results  are  required.    FSPACE  speci-
fies  the  type  of  frequency  spacing  (linear,  logarithmic  or  biased)  to  be 
used.  These frequency points for which results are required can be spaced 
equally along the frequency axis (on a linear or logarithmic scale).  Or they 
can  be  biased  toward  the  eigenfrequencies  (the  frequency  points  are 
placed closer together at eigenfrequencies in the frequency range) so that 
the detailed definition of the response close  to resonance frequencies can 
be obtained. 
b)  The second method is to use a load curve (LCFREQ) to define the frequen-
cies of interest.
*DATABASE_FREQUENCY_BINARY_OPTION 
Options for frequency domain binary output files with the default names given include: 
D3ACC 
D3ACS 
D3ATV 
D3FTG 
D3PSD 
Binary  output  file  for  BEM  acoustics  (element  acoustic  pressure 
contribution  and  contribution  percentage).    See  also  *FREQUEN-
CY_DOMAIN_ACOUSTIC_BEM. 
Binary  output  file  for  FEM  acoustics  (acoustic  pressure  and  sound 
pressure  level).    See  also  *FREQUENCY_DOMAIN_ACOUSTIC_-
FEM. 
Binary  output  file  for  acoustic  transfer  vectors  given  by  BEM 
acoustic analysis.  See also *FREQUENCY_DOMAIN_ACOUSTIC_-
BEM_ATV. 
Binary  output  file  for  random  vibration  fatigue  analysis.    See  also 
*FREQUENCY_DOMAIN_RANDOM_VIBRATION_FATIGUE. 
Binary  Power  Spectral  Density  output  file  for  random  vibration 
analysis.    See  also  *FREQUENCY_DOMAIN_RANDOM_VIBRA-
TION. 
D3RMS 
D3SPCM 
D3SSD 
Binary Root Mean Square output file for random vibration analysis.  
See also *FREQUENCY_DOMAIN_RANDOM_VIBRATION. 
Binary  output  file  for  response  spectrum  analysis.    See  also  *FRE-
QUENCY_DOMAIN_RESPONSE_SPECTRUM. 
Binary  output  file  for steady  state  dynamics.    See  also  *FREQUEN-
CY_DOMAIN_SSD. 
The  D3ACC,  D3ACS,  D3ATV,  D3FTG,  D3PSD,  D3RMS,  D3SPCM  and  D3SSD  files 
contain  plotting  information  to  plot  data  over  the  three  dimensional  geometry  of  the 
model.  These databases can be plotted with LS-PrePost. 
•  The D3PSD file contains PSD state data for a range of frequencies.  The D3SSD 
file contains state data for a range of frequencies. 
•  For D3SSD, the data can be real or complex, depending on the variable BINARY 
defined below. 
•  The  D3ACC  file  contains  acoustic  pressure  contribution  (and  contribution 
percentage)  from  each  of  the  boundary  elements  for  a  range  of  frequencies, 
which are defined in the keyword *FREQUENCY_DOMAIN_ACOUSTIC_BEM. 
•  The D3ACS file contains acoustic results including acoustic pressure and sound 
pressure level for a range of frequencies, which are defined in the keyword *FRE-
QUENCY_DOMAIN_ACOUSTIC_FEM.
•  The  D3FTG,  D3RMS  and  D3SPCM  files  contain  only  one  state  each  as  they  are 
the  data  for  cumulative  fatigue  damage  ratio,  root  mean  square  for  random 
vibration and peak response for response spectrum analysis separately. 
•  The D3ATV file contains NFIELD × NFREQ states, where NFIELD is the number 
of acoustic field points and NFREQ is the number of output frequencies. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BINARY 
Type 
Default 
I 
- 
Remarks 
1 
Additional cards for D3ACC keyword options. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID1 
NID2 
NID3 
NID4 
NID5 
NID6 
NID7 
NID8 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
Additional card for D3PSD and D3SSD keyword options. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FMIN 
FMAX 
NFREQ 
FSPACE 
LCFREQ 
Type 
F 
F 
Default 
0.0 
0.0 
I 
0 
I 
0 
I
VARIABLE   
DESCRIPTION
BINARY 
Flag for writing the binary plot file. 
EQ.0:  Off 
EQ.1:  write the binary plot file  
EQ.2:  write  the  complex  variable  binary  plot  file  (D3SSD
only) 
EQ.90:  write only real part of frequency response (D3SSD only) 
EQ.91:  write  only  imaginary  part  of  frequency  response
(D3SSD only) 
Field  point  node  ID  for  writing  D3ACC  file  (up  to  10  NID  are
allowed) 
Minimum frequency for output (cycles/time) 
Maximum frequency for output (cycles/time). 
NID1,… 
FMIN 
FMAX 
NFREQ 
Number of frequencies for output. 
FSPACE 
Frequency spacing option for output: 
EQ.0:  linear 
EQ.1:  logarithmic 
EQ.2:  biased 
LCFREQ 
Load Curve ID defining the frequencies for output. 
Remarks:
fmin
fmin
fmin
Linear Spacing
Logarithmic Spacing
fmax
fmax
mode n
mode n+1
mode n+2
Biased Spacing
fmax
Figure 14-7.  Spacing options of the frequency points. 
1.  For OPTION = D3SSD, If BINARY = 1, only the magnitude of the displacement, 
velocity,  acceleration  and  stress  response  is  written  into  the  binary  database 
“d3ssd”  which  can  be  accessed  by  LS-PrePost  3.0  or  older  versions.    For  cus-
tomers using LS-PrePost 3.0 or older versions, it is suggested to set BINARY = 
1.  If BINARY = 2, both the magnitude and the phase angle of the response are 
written into “d3ssd” so that LS-PrePost (3.1 or higher versions) can run modal 
expansion (to show the cyclic time history fringe plot) on each output frequen-
cy.  If BINARY = 90 or 91, only real or imaginary part of the response is written 
into “d3ssd”. 
2.  There are two methods to define the output frequencies. 
a)  The first method is to define FMIN, FMAX, NFREQ and FSPACE.  FMIN 
and  FMAX  specify  the  frequency  range  of  interest  and  NFREQ  specifies 
the  number  of  frequencies  at  which  results  are  required.    FSPACE  speci-
fies  the  type  of  frequency  spacing  (linear,  logarithmic  or  biased)  to  be 
used.  These frequency points for which results are required can be spaced 
equally along the frequency axis (on a linear or logarithmic scale).  Or they 
can  be  biased  toward  the  eigenfrequencies  (the  frequency  points  are 
placed closer together at eigenfrequencies in the frequency range) so that 
the detailed definition of the response close  to resonance frequencies can 
be obtained. 
b)  The second method is to use a load curve (LCFREQ) to define the frequen-
cies of interest.
*DATABASE 
Purpose:  When a Lagrangian mesh overlaps with an Eulerian or ALE mesh, the fluid-
structure  (or  ALE-Lagrangian)  interaction  is  often  modeled  using  the  *CON-
STRAINED_LAGRANGE_IN_SOLID  card.    This  keyword  (*DATABASE_FSI)  causes 
certain  coupling  information  related  to  the  flux  through  and  load  on  selected 
Lagrangian  surfaces  defined  in  corresponding  *CONSTRAINED_LAGRANGE_IN_-
SOLID card to be written to the ASCII-based dbfsi file or in the case of MPP-DYNA the 
binout file. 
NOTE:  This  card  must  be  associated  with  a  *CON-
STRAINED_LAGRANGE_IN_SOLID  penalty  meth-
od  coupling.    This  card  is  not  compatible  with 
constrained-based coupling. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DTOUT 
Type 
F 
Surface Card.  Add  one card per surface.  This input terminates at the next keyword 
(“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  DBFSI_ID 
SID 
SIDTYPE 
SWID 
CONVID  NDSETID 
CID 
Type 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
DTOUT 
Output interval time step 
DBFSI_ID 
Surface  ID  (for  reference  purposes  only)  or  a  DATABASE_FSI 
entity  ID.    It  consists  of  a  geometric  entity  defined  by  the  SID
below.
SID 
*DATABASE_FSI 
DESCRIPTION
Set ID defining the geometrical surface(s) through which or upon
which  some  data  is  to  be  tracked  and  output  to  a  file  called
“dbfsi”.    This  set  ID  can  be  a  (1)  PID  or  (2)  PSID  or  (3)  SGSID.
This Lagrangian SID must be contained in a Lagrangian slave SID
defined in a corresponding coupling card, *CONSTRAINED_LA-
GRANGE_IN_SOLID. 
SIDTYPE 
Set type: 
EQ.0: Part set 
EQ.1: Part 
EQ.2: Segment set 
SWID 
CONVID 
This  is  an  ID  from  a  corresponding  *ALE_FSI_SWITCH_MMG_-
ID card.  This card allows for the AMMG ID of an ALE material 
to  be  switched  as  it  passes  across  a  monitoring  surface.    If
defined,  the  accumulative  mass  of  the  “switched”  ALE  multi-
material  group  (AMMG)  is  written  out  under  the  “mout” 
parameter in the “dbfsi” file. 
This is used mostly for airbag application only: CONVID is an ID 
from  a  corresponding  *LOAD_ALE_CONVECTION_ID  card 
which  computes  the  heat  transfer  between  inflator  gas  (ALE
material)  and  the  inflator  canister  (Lagrangian  part).    If  defined,
the temperature of the Lagrangian part having heat transfer with 
the  gas,  and  its  change  in  temperature  as  function  of  time  are
output in the “dbfsi” file. 
NDSETID 
Set ID consisting of the nodes on which the moments of the forces
applied on SID are computed.  See Remark 3. 
CID 
Coordinate system ID, see *DEFINE_COORDINATE_SYSTEM. 
Remarks: 
1.  Overview of dbfsi File.  The dbfsi parameters output are enumerated below. 
pres  =  Averaged estimated coupling pressure over each surface entity 
being monitored.  For example, if using SI base units for mass-
length-time-temperature, this pressure would then be in Pascal.
fx, fy, fz  =  Averaged total estimated coupling force components (N in met-
ric  units)  along  the  global  coordinate  directions,  over  each  sur-
face entity defined, and acting at the centroid of each surface. 
mout  =  Accumulated  mass  (Kg  in  metric  units)  passing  through  each 
DBFS_ID surface entity.  See Remark 2 below.  (This parameter 
used to be called “pleak”). 
obsolete  =  (This parameter used to be called “mflux”). 
  gx, gy, gz  =  Average  estimated  leakage-control  force  component  over  the 
surface entity.  This data is useful for debugging.  Leakage con-
trol forces are too large (relative to the main coupling forces, fx, 
fy and fz) may indicate that alternate coupling approach should 
be  considered  since  the  main  coupling  force  is  putting  out  too 
little resistance to leakage.  (These parameters used to be called 
fx-lc, fy-lc and fz-lc). 
Ptmp  =  Lagrangian  part  Temperature  (Activated  only  when  the 
*LOAD_ALE_CONVECTION card is used). 
PDt  =  Lagrangian part Temperature change (Activated only when the 
*LOAD_ALE_CONVECTION card is used). 
2.  MOUT.    “mout”  parameter  in  the  “dbfsi”  output  from  this  keyword  contains 
the  accumulated  mass  passing  through  each  DBFS_ID  surface  entity.    For  4 
different cases: 
a)  When  LCIDPOR  is  defined  in  the  coupling  card  (CLIS),  porous  accumu-
lated mass transport across a Lagrangian shell surface may be monitored 
and output in “mout”. 
b)  Porous flow across Lagrangian shell may also be defined via a load curve 
in the *MAT_FABRIC card, and similar result will be tracked and output.  
This is an alternate form of (a). 
c)  When NVENT in the CLIS card is defined (isentropic venting), the venting 
mass  transport  across  the  isentropic  vent  hole  surface  may  be  output  in 
“mout”. 
d)  When  an  *ALE_FSI_SWITCH_MMG_ID  card  is  defined,  and  the  SWID 
parameter specifies this ID to be tracked, then the amount of accumulated 
mass that has been switched when passing across a monitoring surface is 
output.
3.  Calculation  of  Moments  for  NDSETID.    A  geometrical  surface  SID  has  a 
centroid  where  the  coupling  forces  are  averaged.    The  distances  between  this 
centroid  and  the  nodes  defined  by  the  set  NDSETID  are  the  lever  arms.    The 
moments are the cross-products of these distances with the averaged coupling 
forces.  For each node in the set NDSETID,  a new line in the “dbfsi” file is in-
serted after each output for the corresponding coupling forces .  
These  additional  lines  have  the  format  following  the  template  established  by 
the example in Remark 1 where the forces are replaced by the moments and the 
node ID replaces the DBFSI_ID values. 
Example: 
Consider a model with a Lagrangian mesh overlaps with an Eulerian or ALE mesh.  On 
the Lagrangian mesh, there are 3 Lagrangian surface sets over which some data is to be 
written out. 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
$ INPUT: 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
*DATABASE_FSI 
$       dt 
  2.97E-06 
$ DBFSI_ID       SID     STYPE      swid    convid [STYPE: 0=PSID;1=PID;2=SGSID] 
        11         1         2 
        12         2         2 
        13         3         1  
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
$ This reads: 
$ DBFSI_ID 11 is defined by a SID=1: a SGSID = as specified by STYPE=2 
$ DBFSI_ID 12 is defined by a SID=2: a SGSID = as specified by STYPE=2 
$ DBFSI_ID 13 is defined by a SID=3: a PID   = as specified by STYPE=1 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
$ An OUTPUT file called “dbfsi” looks like the following: 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
     Fluid-structure interaction output  
     Number of surfaces:       3 
        id          pres            fx            fy            fz          mout 
                obsolete            gx            gy            gz          Ptmp          
PDt 
         time=  0.00000E+00 
        11    0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00 
              0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00     
0.0000E+00 
        12    0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00 
              0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00     
0.0000E+00 
        13    0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00 
              0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00     
0.0000E+00 
         time=  0.29709E-05 
        11    0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00 
              0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00     
0.0000E+00
12    0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00 
              0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00     
0.0000E+00 
        13    0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00 
              0.1832E-06    0.0000E+00    0.0000E+00    0.0000E+00    0.0000E+00     
0.0000E+00 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8
*DATABASE_FSI_SENSOR 
Purpose:    This  card  activates  the  output  of  an  ASCII  file  called  “dbsensor”.    Its  input 
defines  the  pressure  sensors’  locations  which  follow  the  positions  of  some  Lagrangian 
segments  during  the  simulation.    Its  ASCII  output  file,  dbsensor,  contains  the  spatial 
position of the sensor and its recorded pressure from the ALE elements containing the 
sensors.  This card is activated when a *CONSTRAINED_LAGRANGE_IN_SOLID card 
is used and the Lagrangian shell elements defining the locations of the sensors must be 
included in the slave or structure coupling set. 
2 
3 
4 
5 
6 
7 
8 
  Card 1 
Variable 
1 
DT 
Type 
F 
Surface Card.  Add  one card per surface.    This input terminates  at the next keyword 
(“*”) card. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  DBFSI_ID 
NID 
SEGMID 
OFFSET 
ND1 
ND2 
ND3 
Type 
I 
I 
I 
F 
I 
I 
I 
  VARIABLE   
DESCRIPTION
DT 
Output interval 
DBFSI_ID 
Pressure-Sensor ID. 
NID 
SEGMID 
An  optional  Lagrangian  node  ID  defining  an  approximate
pressure  sensor  location  with  respect  to  a  Lagrangian  shell
element.  This is not a required input. 
A  required  Lagrangian  element  ID  for  locating  the  pressure
sensor.    If  NID = 0  or  blank,  the  sensor  will  be  automatically 
placed  in  the  center  of  this  SEGMID,  accounting  for  the  offset
distance.    If  the  model  is  3D,  the  Lagrangian  element  can  be  a
shell or solid (for this latter, ND1 and ND2 are required to define
the  face).    If  the  model  is  2D,  the  Lagrangian  element  can  be  a 
beam or shell (for this latter, ND1 and ND2 are required to define
the side).
DESCRIPTION
Offset  distance  between  the  pressure  sensor  and  the  Lagrangian
segment surface.  If it is positive, it is on the side pointed to by the
segment normal vector and vice versa. 
Nodes  defining  the  solid  face  in  3D  or  shell  side  in  2D,  from
which  the  sensor  is  located.    In  3D,  if the  solid  face  has  4  nodes,
only  the  diagonal  opposites  ND1  and  ND2  are  required.    If  the
solid face is triangular, a third node ND3 should be provided.  In
2D, only ND1 and ND2 are required to define the shell side. 
  VARIABLE   
OFFSET 
ND1, ND2, 
ND3 
Remarks: 
1.  The output parameters in the “dbsensor” ASCII file are: 
ID  =  Sensor ID.  
  x, y, z  =  Sensor spatial location. 
P  =  Sensor recorded pressure (Pa) from the ALE fluid element con-
taining the sensor. 
For example, to plot the sensor pressure in LS-Prepost, select: 
ASCII → dbsensor → LOAD → (select sensor ID) → Pressure → PLOT 
Example 1: 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
$ INPUT: 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
*DATABASE_FSI_SENSOR 
      0.01 
$ DBFSI_ID       NID SEGMENTID    OFFSET 
        10       360       355      -0.5 
        20       396       388      -0.5 
        30       324       332      -0.5 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
$ The 1st line reads: 
$ SENSOR_ID 10 is located by segment-ID=355.  Node-ID=360 precisely locate this  
$ sensor (if NID=0, then the sensor is located at the segment center).  This 
$ sensor is located 0.5 length unit away from the segment surface.  Negative  
$ sign indicates a direction opposite to the segment normal vector. 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
$ An OUTPUT file called “dbsensor” looks like the following: 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
     ALE sensors output  
     Number of sensors:  3 
        id          x            y             z             p     
         time=  0.17861E-02 
        10    0.0000E+00    0.0000E+00   -0.3900E+00    0.1085E-03
20   -0.2250E+02    0.2250E+02   -0.3900E+00    0.1085E-03 
        30    0.2250E+02   -0.2250E+02   -0.3900E+00    0.1085E-03 
         time=  0.20081E-02 
        10    0.0000E+00    0.0000E+00   -0.3900E+00    0.1066E-03 
        20   -0.2250E+02    0.2250E+02   -0.3900E+00    0.1066E-03 
        30    0.2250E+02   -0.2250E+02   -0.3900E+00    0.1066E-03 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
$ ID    = DBFSI_ID 
$ x,y,z = Sensor location (defined based on a Lagrangian segment)  
$ p     = Sensor pressure as taken from the fluid element containing the sensor. 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8
Available options include: 
*DATABASE 
BEAM 
BEAM_SET 
BEAM_ID 
DISCRETE 
DISCRETE_ID 
DISCRETE_SET 
NODE 
NODE_ID 
NODE_LOCAL 
NODE_LOCAL_ID 
NODE_SET 
NODE_SET_LOCAL 
SEATBELT 
SEATBELT_ID 
SHELL 
SHELL_ID 
SHELL_SET 
SOLID 
SOLID_ID 
SOLID_SET 
SPH 
SPH_SET 
TSHELL 
TSHELL_ID
*DATABASE_HISTORY 
Purpose:    Control  which  nodes  or  elements  are  output  into  the  binary  history  file, 
d3thdt, the ASCII file nodout, the ASCII file elout and the ASCII file sphout.  Define as 
many  cards  as  necessary.    The  next  “*”  card  terminates  the  input.    See  also  *DATA-
BASE_BINARY_OPTION and *DATABASE_OPTION. 
Node/Element  Cards  for  Case  I  (no  “ID”,  and  no  “LOCAL”).    Cards  for  keyword 
options  BEAM,  BEAM_SET,  DISCRETE,  DISCRETE_SET,  NODE,  NODE_SET,  SEAT-
BELT,  SHELL,  SHELL_SET,  SOLID,  SOLID_SET,  SPH,  SPH_SET,  TSHELL,  and 
TSHELL_SET.  Include as many as needed.  Input terminates at the next keyword (“*”) 
card. 
  Card 1 
1 
Variable 
ID1 
2 
ID2 
3 
ID3 
4 
ID4 
5 
ID5 
6 
ID6 
7 
ID7 
8 
ID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
IDn 
DESCRIPTION
NODE/NODE_SET or element/element set ID n.  Elements may 
be  BEAM/BEAM_SET,  DISCRETE/DISCRETE_SET,  SEATBELT, 
TSHELL/
SHELL/SHELL_SET, 
TSHELL_SET.  The contents of the files are given in Table 14-2 for 
nodes,  Table  14-3  for  solid  elements,  Table  14-4  for  shells  and 
thick shells, and Table 14-5 for beam elements.  In the binary file, 
D3THDT,  the  contents  may  be  extended  or  reduced  with  the 
*DATABASE_EXTENT_BINARY definition. 
SOLID/SOLID_SET, 
or 
Node/Element Cards for Case II (“ID” option, but no “LOCAL”).  Cards for keyword 
options BEAM_ID, NODE_ID, SEATBELT_ID, SHELL_ID, SOLID_ID, and TSHELL_ID. 
Include as many as needed.  Input terminates at the next keyword (“*”) card. 
  Card 1 
Variable 
1 
ID 
Type 
I 
2 
3 
4 
5 
6 
7 
8 
HEADING 
A70 
  VARIABLE   
DESCRIPTION
ID 
Node or element ID
VARIABLE   
HEADING 
DESCRIPTION
A description of the node or element.  It is suggested that unique
descriptions be used.  This description is written into the D3HSP
file and into the ASCII databases nodout and elout. 
Node Cards for Case III (“LOCAL” option).  Card 1 for keyword options NODE_LO-
CAL, NODE_LOCAL_ID, and NODE_SET_LOCAL.  Include as many cards as needed 
to specify all the nodes.  This input terminates at the next keyword (“*”) card. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
CID 
REF 
HFO 
Type 
I 
I 
I 
I 
ID  Card  for  Case  III.    Additional  card  for  ID  option.    This  card  is  only  used  for  the 
NODE_LOCAL_ID keyword option.  When activated, each node is specified by a pair 
of  cards  consisting  of  “Card  1,”  and,  secondly,  this  card.    Include  as  many  pairs  as 
needed to specify all the nodes.  This input terminates at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
HEADING 
A70 
  VARIABLE   
DESCRIPTION
ID 
CID 
NODE/NODE_SET set ID.  The contents of the files are given in 
Table  14-2  for  nodes. 
  See  the  remark  below  concerning
accelerometer nodes. 
Coordinate  system  ID  for  nodal  output.    See  DEFINE_COORDI-
NATE options.
REF 
*DATABASE_HISTORY 
DESCRIPTION
Output  coordinate  system  for  displacements,  velocities,  and
accelerations.    (Nodal  coordinates  are  always  in  the  global
coordinate system.) 
EQ.0:  Output  is  in  the  local  system  fixed  for  all  time  from  the 
beginning of the calculation.  If CID is nonzero, FLAG in
the  corresponding  *DEFINE_COORDINATE_NODES 
command  must  be  set  to  0.    FLAG  has  no  bearing  on
results when REF is set to 1 or 2. 
EQ.1:  Translational  output  is  the  projection  of  the  node’s 
absolute translational motion onto the local system.  The
local  system  is  defined  by  the  *DEFINE_COORDI-
NATE_NODES  command  and  can  change  orientation
according  to  the  movement  of  the  three  defining  nodes.
The  defining  nodes  can  belong  to  either  deformable  or 
rigid parts.  
EQ.2:  Translational  output  is  the  projection  of  the  node’s
relative translational motion onto the local system.  Here,
“relative” means relative to node N1 of that local system.
In other words, the displacement of the origin (node N1) 
of the local coordinate system is first subtracted from the
displacement  of  the  node  of  interest  before  projecting  it
onto the translating and rotating local coordinate system.
The  local  system  is  defined  as  described  in  REF = 1
above.  If dynamic relaxation is used, the reference loca-
tion  is  reset  when  convergence  is  achieved.    Rotational
output  is  truly  relative  to  the  updated  location  coordi-
nate system only if REF = 2.  
HFO 
Flag for high frequency output into nodouthf 
EQ.0:  Nodal data written to nodout file only 
EQ.1:  Nodal data also written nodouthf at the higher frequency
HEADING 
A  description  of  the  nodal  point.    It  is  suggested  that  unique
description  be  used.    This  description  is  written  into  the  d3hsp
file and into the ASCII database nodout. 
Remarks: 
1. 
If  a  node  belongs  to  an  accelerometer,  see  *ELEMENT_SEATBELT_AC-
CELEROMETER, and if it also appears as an active node in the NODE_LOCAL
or NODE_SET_LOCAL keyword, the coordinate system, CID, transformations 
will be skipped and the LOCAL option will have no effect.
*DATABASE_MASSOUT 
Purpose:  Output nodal masses into ASCII file MASSOUT. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SETID 
NDFLG 
RBFLG 
Type 
Default 
I 
0 
I 
1 
I 
0 
  VARIABLE   
DESCRIPTION
SETID 
Optional set ID. 
EQ.0:  mass output for all nodes, 
LT.0:  no output, 
GT.0:  set ID identifying nodes whose mass will be output. 
NDFLG 
Database extent: 
EQ.1:  output 
translational  mass 
identified by SETID (default), 
for  deformable  nodes
EQ.2:  output  translational  mass  and  rotary  inertias  for  the
deformable nodes identified by the SETID.  
EQ.3:  output  translational  mass  for  deformable  and  rigid
nodes identified by SETID (default), 
EQ.4:  output  translational  mass  and  rotary  inertias  for  the
deformable and rigid nodes identified by the SETID. 
RBFLG 
Rigid body data: 
EQ.0:  no output for rigid bodies, 
EQ.1:  output rigid body mass and inertia. 
Remarks: 
1.  Nodes  and  rigid  bodies  with  no  mass  are  not  output.   By  inference,  when  the 
set ID is zero and no output shows up for a node, then the mass of that node is 
zero.
*DATABASE_NODAL_FORCE_GROUP 
Purpose:  Define a nodal force group for output into the ASCII file nodfor.  The output 
interval must be specified using *DATABASE_NODFOR . 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSID 
CID 
Type 
I 
I 
Default 
none 
none 
  VARIABLE   
DESCRIPTION
Nodal set ID, see *SET_NODE_OPTION. 
Coordinate system ID for output of data in local system, 
NSID 
CID 
Remarks: 
1.  The  reaction  forces  in  the  global  𝑥,  𝑦,  and  𝑧  directions  (and  local  𝑥,  𝑦,  and  𝑧 
directions if CID is defined above) for the nodal force group are written to the 
nodfor file  along with the external work done by 
these reaction forces.  The reaction forces in the global 𝑥, 𝑦, and 𝑧 directions for 
each node in the nodal force group are also written to nodfor.  These forces can 
be a result of applied boundary forces such as nodal point forces and pressure 
boundary conditions, body forces, and contact interface forces.  In the absence 
of body forces, interior nodes would always yield a null force resultant vector.  
In general this option would be used for surface nodes.
*DATABASE_PAP_OUTPUT 
Purpose:  Set contents of output files for pore air pressure calculations. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IVEL 
IACCX 
IACCY 
IACCZ 
NCYOUT 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
100 
  VARIABLE   
DESCRIPTION
IVEL 
Meaning of “Velocity” in d3plot and d3thdt output files 
EQ.0:  Nodal velocity vector 
EQ.1:  Seepage velocity vector 
IACCX, Y, Z 
Meaning  of  “X/Y/Z-Acceleration”  in  d3plot  and  d3thdt  output 
files 
EQ.0:  Not written 
EQ.21:  Nodal air density 
EQ.22:  Nodal pore air pressure 
EQ.24:  Nodal air mass 
EQ.25:  Nodal air mass flow rate 
NCYOUT 
Number of cycles between outputs of calculation status to d3hsp
and log files
*DATABASE 
Purpose:  Plot the distribution or profile of a data along x, y, or z-direction. 
  Card 1 
Variable 
1 
DT 
Type 
I 
2 
ID 
I 
3 
4 
5 
6 
7 
8 
TYPE 
DATA 
DIR 
UPDLOC 
MMG 
I 
I 
I 
I 
0 
I 
0 
Default 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
DT 
ID 
Interval time. 
Set ID. 
TYPE 
Set type: 
EQ.1:  Node Set, 
EQ.2:  Solid Set, 
EQ.3:  Shell Set, 
EQ.4:  Segment Set, 
EQ.5:  Beam Set. 
DATA 
Data type: 
EQ.1:  𝑥-velocity, 
EQ.2:  𝑦-velocity, 
EQ.3:  𝑧-velocity, 
EQ.4:  velocity magnitude, 
EQ.5:  𝑥-acceleration, 
EQ.6:  𝑦-acceleration, 
EQ.7:  𝑧-acceleration, 
EQ.8:  acceleration magnitude, 
EQ.9:  pressure, 
EQ.10:  𝑥𝑥-stress,
VARIABLE   
DESCRIPTION
EQ.11:  𝑦𝑦-stress, 
EQ.12:  𝑧𝑧-stress, 
EQ.13:  𝑥𝑦-stress, 
EQ.14:  𝑦𝑧-stress, 
EQ.15:  𝑧𝑥-stress, 
EQ.16:  temperature, 
EQ.17:  volume fraction, 
EQ.18:  kinetic energy, 
EQ.19:  internal energy, 
EQ.20:  density. 
DIR 
Direction: 
EQ.1:  𝑥-direction, 
EQ.2:  𝑦-direction, 
EQ.3:  𝑧-direction,  
EQ.4:  Curvilinear  (relative  distances  between  elements  of  set
ID are added up in the order defined by the set) 
UPDLOC 
Flag to update the set location: 
EQ.0:  Only the initial position of set ID is considered 
EQ.1:  The  positions  of  the  elements  composing  the  set  are
updated each DT 
MMG 
Multi-Material ALE group id.  See Remark 2. 
GT.0:  Multi-Material ALE group id 
LT.0:  |MMG|  is  the  id  of  a  *SET_MULTI-MATERIAL_-
GROUP_LIST  that  can  list  several  Multi-Material  ALE 
group ids. 
Remarks: 
1.  At  a  given  time  𝑇  the  profile  is  written  in  a  file  named  profile_DATA_-
DIR_timeT.xy  (DATA  and  DIR  are  replaced  by  the  data  and  direction  names 
respectively).    The  file  has  a  xyplot  format  that  LS-PrePost  can  read  and  plot.  
For example, DATA = 9, DIR = 2 and DT = 0.1 sec will save a pressure profile at
𝑡 = 0.0 sec in profile_pressure_y_time0.0.xy, at 𝑡 = 0.1 sec in profile_pressure_y_
time0.1.xy, at 𝑡 = 0.2 sec in profile_pressure_y_time0.2.xy. 
2. 
In the case of a multi-material ALE model (elform = 11 in *SECTION_SOLID or 
*SECTION_ALE2D  or  *SECTION_ALE1D),  an  element  can  contain  several 
materials  with  each  material  being  associated  with  its  own  pressures  and 
stresses.    It  is  the  default  behavior  for  volume  averaging  to  be  applied  to  ele-
ment  data  before  being  written  out;  however,  when  the  multi-material  group 
field, MMG, is set, then element data are output only for the specified materials.
*DATABASE_PWP_FLOW 
Purpose:  Request output containing net inflow of fluid at a set of nodes. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSET 
Type 
Default 
I 
0 
  VARIABLE   
DESCRIPTION
NSET 
Node set ID 
Remarks: 
Any  number  of  these  cards  can  be  used.    Nett  inflow  or  outflow  arises  when 
maintaining an applied PWP boundary condition implies addition or removal of water. 
Output is written to a file named database_pwp_flow.csv, a comma-separated ascii file.  
Each line consists of (time, flow1, flow2, …) where flow1 is the total inflow at the node 
set for the first DATABASE_PWP_FLOW request, flow2 is for the second, etc.
*DATABASE 
Purpose:  Set contents of output files for pore pressure calculations. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IVEL 
IACCX 
IACCY 
IACCZ 
NCYOUT 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
100 
  VARIABLE   
DESCRIPTION
IVEL 
Meaning of “Velocity” in d3plot and d3thdt output files 
EQ.0:  Nodal velocity vector 
EQ.1:  Seepage velocity vector 
IACCX, Y, Z 
Meaning  of  “X/Y/Z-Acceleration”  in  d3plot  and  d3thdt  output 
files 
EQ.0:  Not written 
EQ.1:  Total pwp head 
EQ.2:  Excess pwp head (this is also written as temperature) 
EQ.3:  Target rate of volume change 
EQ.4:  Actual rate of volume change 
EQ.7:  Hydraulic pwp head 
EQ.8:  Error  in  rate  of  volume  change  (calculated  from
seepage minus actual) 
EQ.9:  Volume at node 
EQ.10:  Rate of volume change calculated from seepage 
EQ.14:  Void volume (generated at suction limit) 
EQ.17:  NFIXCON (e.g: +4/-4 for nodes on suction limit) 
NCYOUT 
Number  of  cycles  between  outputs  of  calculation  status  to
d3hsp,  log,  and  tdc_control_output.csv  files  (time-dependent 
and steady-state analysis types).
*DATABASE_RCFORC_MOMENT 
Purpose:  Define contact ID and nodes for moment calculations.  Moments are written 
to  rcforc  according  to  output  interval  given  in  *DATABASE_RCFORC.    If  *DATA-
BASE_RCFORC_MOMENT  is  not  used,  the  moments  reported  to  rcforc  are  about  the 
origin (0, 0, 0).  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CID 
NODES 
NODEM 
Type 
I 
I 
I 
  VARIABLE   
DESCRIPTION
CID 
Contact ID 
NODES 
NODEM 
Node  about  which  moments  are  calculated  due  to  contact  forces
on slave surface.   
Node  about  which  moments  are  calculated  due  to  contact  forces 
on master surface.
*DATABASE 
Purpose:  Recovers the stresses at nodal points of solid or thin shell elements by using 
Zienkiewicz-Zhu’s Superconvergent Patch Recovery method.  
5 
6 
7 
8 
  Card 1 
1 
Variable 
PSID 
Type 
Default 
I 
0 
2 
IAX 
A 
0 
3 
IAY 
A 
0 
4 
IAZ 
A 
0 
  VARIABLE   
PSID 
DESCRIPTION
Part set ID of solid or thin shell elements whose nodal stress will
be recovered 
IAX, IAY, IAZ 
Meaning  of  “𝑥/𝑦/𝑧-Acceleration”  in  d3plot  and  d3thdt  output 
files 
EQ.SMNPD:  the minimum principal deviator stress 
EQ.SMNPR:  the minimum principal stress 
EQ.SMXPD:  the maximum principal deviator stress 
EQ.SMXPR:  the maximum principal stress 
EQ.SMXSH:  the maximum shear stress 
EQ.SPR: 
nodal pressure 
EQ.SVM: 
nodal von Mises stress 
EQ.SXX: 
EQ.SYY: 
EQ.SZZ: 
EQ.SXY: 
EQ.SYZ: 
EQ.SZX: 
nodal normal stress along 𝑥 direction 
nodal normal stress along 𝑦 direction 
nodal normal stress along 𝑧 direction 
nodal shear stress along 𝑥-𝑦 direction 
nodal shear stress along 𝑦-𝑧 direction 
nodal shear stress along 𝑧-𝑥 direction 
For shell elements append either “B” or “T” to the input string to
recover  nodal  stresses  at  the  bottom  or  top  layer  of  shell 
elements.  For example, SPRT recovers the nodal pressure at the
top layer.
*DATABASE_RECOVER_NODE 
1.  Recovered stresses are in global coordinate system.
*DATABASE_SPRING_FORWARD 
Purpose:    Create  spring  forward  nodal  force  file.    This  option  is  to  output  resultant 
nodal  force  components  of  sheet  metal  at  the  end  of  the  forming  simulation  into  an 
ASCII file, “SPRING-FORWARD”, for spring forward and die corrective simulations. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IFLAG 
Type 
I 
  VARIABLE   
DESCRIPTION
IFLAG 
Output type: 
EQ.0:  off, 
EQ.1:  output element nodal force vector for deformable nodes.
*DATABASE_SUPERPLASTIC_FORMING 
Purpose:    Specify  the  output  intervals  to  the  superplastic  forming  output  files.    The 
option *LOAD_SUPERPLASTIC_FORMING must be active. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DTOUT 
Type 
F 
  VARIABLE   
DTOUT 
DESCRIPTION
Output  time  interval  for  output  to  “pressure”,  “curve1”  and
“curve2”  files.    The  “pressure”  file  contains  general  information
from  the  analysis  and  the  files  “curve1”  and  “curve2”  contain
pressure  versus  time  from  phases  1  and  2  of  the  analysis.    The
data in the pressure and curve files may be plotted using ASCII →
superpl in LS-PrePost.
*DATABASE 
Purpose:  Tracer particles will save a history of either a material point or a spatial point 
into  an  ASCII  file:  trhist.    This  history  includes  positions,  velocities,  and  stress 
components.  The option *DATABASE_TRHIST must be active.  This option applies to 
ALE, SPH and DEM (Discrete Element Method) problems. 
Available options are: 
<BLANK> 
DE 
The  DE  option  defines  a  tracer  corresponding  to  discrete  elements  (*ELEMENT_DIS-
CRETE_SPHERE) .  See Remarks 2 and 4. 
Card 
1 
2 
Variable 
TIME 
TRACK 
Type 
F 
Default 
0.0 
I 
0 
3 
X 
F 
0 
4 
Y 
F 
0 
5 
Z 
F 
0 
6 
7 
8 
AMMGID 
NID 
RADIUS 
I 
0 
I 
0 
F 
0.0 
  VARIABLE   
DESCRIPTION
TIME 
Start time for tracer particle 
TRACK 
Tracking option: 
EQ.0:  particle follows material, 
EQ.1:  particle is fixed in space. 
X 
Y 
Z 
Initial 𝑥-coordinate 
Initial 𝑦-coordinate 
Initial 𝑧-coordinate 
AMMGID 
The AMMG ID (ALE multi-material group) of the material being 
tracked in a multi-material ALE element.  See Remark 1.
NID 
*DATABASE_TRACER 
DESCRIPTION
An  optional  node  ID  defining  the  initial  position  of  a  tracer
particle.    If  defined,  its  coordinates  will  overwrite  the  𝑥,  𝑦,  𝑧
coordinates above.  This feature is for TRACK = 0 only and can be 
applied to ALE tracers and DE tracers.  See Remark 2. 
RADIUS 
Radius  is  used  only  for  the  DE  option  to  indicate  whether  the
tracer follows and monitors a single discrete element or multiple 
discrete elements. 
GT.0:  The  tracer  takes  the  average  results  of  all  discrete
elements located inside a sphere with radius = RADIUS. 
That sphere stays centered on the DE tracer. 
LT.0:  The  discrete  element  closest  to  the  tracer  is  used.    The 
magnitude of RADIUS in this case is unimportant. 
Remarks: 
1.  Multi-Material  Groups.    ALE  elements  can  contain  multi-materials.    Each 
material is referred to as an ALE multi-material group or AMMG.  Each AMMG 
has its list of history variables that can be output.  For example, if a tracer is in a 
mixed element consisting of 2 AMMGs, and the history variables  of AMMG 1 
are to be output or tracked, the AMMGID should be defined as AMMGID=1.  If 
AMMGID=0,  a  volume-fraction-weighted-averaged  pressure  will  be  reported 
instead. 
2.  NID Description.   For ALE, NID is a massless dummy node.  Its location will 
be updated according to the motion of the ALE material. 
For the DE option, NID is a discrete element node that defines the initial loca-
tion of the tracer.  The DE tracer continues to follow that node if RADIUS < 0.  
On the other hand, the DE tracer’s location is updated according to the average 
motion  of the group of  DE  nodes  inside  the  sphere  defined  by  RADIUS  when 
RADIUS > 0.   
3.  Tracer  particles  in  ambient  ALE  elements.  Since  the  auxiliary  variables  (6 
stresses,  plastic  strain,  internal  energy,  …)  for  ambient  elements  are  reset  to 
their initial values before and after advection and tracer data are stored in trhist 
during the advection cycle, tracers in ambient elements show the initial stresses, 
not the current ones. 
4.  Discrete Elements.  If _DE is used, tracer particles will save a history of either 
a  material  point  or  a  spatial  point  into  an  ASCII  file:  demtrh.    This  history  in-
cludes positions, velocities components, stress components, porosity, void ratio, 
and coordination number.  The option *DATABASE_TRHIST must be active.
*DATABASE_TRACER_GENERATE  
Purpose:    Generate  tracer  particles  along  an  isosurface  for  a  variable  defined  in  the 
VALTYPE  list.    The  tracer  particles  follow  the  motion  of  this  surface  and  save  data 
histories into a binary file called trcrgen_binout .  These histories 
are  identical  to  the  ones  output  by  *DATABASE_TRACER  into  the  trhist  file.    They 
include  positions,  velocities,  and  stress  components.    Except  for  the  positions  and 
element  id  specifying  where  the  tracer  is,  the  output  can  be  controlled  with  the 
VARLOC and VALTYPE2 fields.  This option applies to ALE problems. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DT 
VALOW 
VALUP 
VALTYPE1
SET 
SETYPE  MMGSET 
UPDT 
Type 
F 
F 
F 
I 
Default 
none 
0.0 
0.0 
none 
I 
0 
I 
0 
I 
F 
none 
0.0 
Optional  Variable  Cards.  Cards  defining  new  variables  to  be  output  to  t
trcrgen_binout  instead  of  the  default  ones.    Include  as  many  cards  as  necessary.    This 
input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VARLOC  VALTYPE2  MMGSET
Type 
Default 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DT 
VALOW, 
VALUP 
DESCRIPTION
Interval  time  between  each  tracer  generation  and  position
update . 
Range  of  values  between  which  the  isosurface  is  defined.
VALOW is the lower bound while VALUP is the upper bound.
See  Remark  2.    The  value  at  the  isosurface  is  0.5(VALOW +
VALUP). 
  The  variable  with  this  value  is  defined  by
VALTYPE.
VARIABLE   
VALTYPE1 
VALTYPE2 
DESCRIPTION
The variable that will be used to generate the isosurfaces.  See
VALTYPE2 for enumeration of values. 
Data to be output to the trcrgen_binout file.  The interpretation 
of VALTYPE1 and VALTYPE2 is enumerated in the following
list: 
EQ.1: 
EQ.2: 
EQ.3: 
EQ.4: 
EQ.5: 
EQ.6: 
EQ.7: 
EQ.8: 
EQ.9: 
EQ.10: 
𝑥𝑥-stress  
𝑦𝑦-stress  
𝑧𝑧-stress  
𝑥𝑦-stress  
𝑦𝑧-stress  
𝑧𝑥-stress  
plastic strain  
internal energy  
bulk viscosity  
relative volume  
GE.11 and LE.19: 
other auxiliary variables  
EQ.20: 
EQ.21: 
EQ.22: 
EQ.23: 
EQ.24: 
EQ.25: 
EQ.26: 
EQ.27: 
EQ.28: 
EQ.29: 
EQ.30: 
EQ.31: 
EQ.31: 
EQ.33: 
EQ.34: 
pressure  
density  
material volume  
compression ratio 
element volume fraction 
nodal volume fraction 
𝑥-position 
𝑦-position 
𝑧-position 
𝑥-velocity 
𝑦-velocity 
𝑧-velocity 
velocity 
𝑥-acceleration 
𝑦- acceleration
*DATABASE_TRACER_GENERATE 
EQ.35: 
EQ.36: 
EQ.37: 
EQ.38: 
DESCRIPTION
𝑧- acceleration 
acceleration 
nodal mass 
nodal temperature 
SET 
Set ID  
SETYPE 
Type of set : 
EQ.0: 
EQ.1: 
EQ.2: 
solid set  
segment set  
node set  
MMGSET 
Multi-material group set .  
UPDT 
Time interval between tracer position update . 
VARLOC 
Variable  location  in  trcrgen_binout  to  be  replaced  with  the 
variable specified in the VALTYPE2 field: 
EQ.4: 
EQ.5: 
EQ.6: 
EQ.7: 
EQ.8: 
EQ.9: 
EQ.10: 
EQ.11: 
EQ.12: 
EQ.13: 
EQ.14: 
EQ.15: 
𝑥-velocity 
𝑦-velocity  
𝑧-velocity 
𝑥𝑥-stress  
𝑦𝑦-stress  
𝑧𝑧-stress  
𝑥𝑦-stress  
𝑦𝑧-stress  
𝑧𝑥-stress  
plastic strain  
density  
relative volume  
Remarks: 
1.  DT.    The  frequency  to  create  tracers  is  defined  by  DT.    The  default  value  of 
UPDT, which is the time interval between updates to the tracer position, is also
set to DT.  The default behavior, then, is to update tracer positions when a new 
tracer is created, however, by setting UPDT to a value less than DT tracer posi-
tions can be updated more frequently without creating new tracers.  
2.  Tracing Algorithm.  When LS-DYNA adds new tracer particles  tracers 
are created at element centers, segment centers, or nodes depending on the set 
type (SETYPE).  A new tracer particle is created when the value at the element 
center,  segment  center,  or  node  center  is  in  the  bounding  interval  [VALOW, 
VALUP], provided that there is not already a nearby tracer particle.  The tracer 
particles follow the iso-surface defined by the midpoint of the bounding inter-
val (VALOW + VALUP)/2. 
3.  Multi-Material  Groups.    ALE  elements  can  contain  several  materials.    Each 
material  is  referred  to  as  an  ALE  multi-material  group.    The  volume  fractions 
define how much of the element volume is occupied by the groups.  Each group 
has their own variables for 0<VALTYPE<26.  IF VALTYPE<21 or VALTYPE=23, 
the variable is volume averaged over the groups defined by MMGSET. 
4.  Post-Procesing.  The output of *DATABASE_TRACER_GENERATE is written 
to a file named trcrgen_binout.  To access the output in LS-PrePost: [TAB 2] → 
[LOAD] → [trcrgen_binout] → [trhist] → “Trhist Data” window contains a list of 
variables output for each tracer.  
5.  Binary  to  ASCII  File  Conversion.    The  variables  in  trhist  and  trcrgen_binout 
are  arranged  in  an  identical  order.    Therefore,  the  trhist  can  be  obtained  from 
the trcgen_binout file by using the l2a program located at http://ftp.lstc.com/-
user/lsda. 
.
The  keyword  *DEFINE  provides  a  way  of  defining  boxes,  coordinate  systems,  load 
curves,  tables,  and  orientation  vectors  for  various  uses.    The  keyword  cards  in  this 
section are defined in alphabetical order: 
*DEFINE_ADAPTIVE_SOLID_TO_DES 
*DEFINE_ADAPTIVE_SOLID_TO_SPH 
*DEFINE_BOX 
*DEFINE_BOX_ADAPTIVE 
*DEFINE_BOX_COARSEN 
*DEFINE_BOX_DRAWBEAD 
*DEFINE_BOX_SPH 
*DEFINE_CONNECTION_PROPERTIES_{OPTION} 
*DEFINE_CONSTRUCTION_STAGES 
*DEFINE_CONTACT_EXCLUSION 
*DEFINE_CONTACT_VOLUME 
*DEFINE_COORDINATE_NODES 
*DEFINE_COORDINATE_SYSTEM 
*DEFINE_COORDINATE_VECTOR 
*DEFINE_CPM_BAG_INTERACTION 
*DEFINE_CPM_CHAMBER 
*DEFINE_CPM_GAS_PROPERTIES 
*DEFINE_CPM_VENT 
*DEFINE_CRASHFRONT 
*DEFINE_CURVE_{OPTION} 
*DEFINE_CURVE_BOX_ADAPTIVITY
*DEFINE_CURVE_DRAWBEAD 
*DEFINE_CURVE_DUPLICATE 
*DEFINE_CURVE_ENTITY 
*DEFINE_CURVE_FEEDBACK 
*DEFINE_CURVE_FLC 
*DEFINE_CURVE_FUNCTION 
*DEFINE_CURVE_SMOOTH 
*DEFINE_CURVE_TRIM_{OPTION} 
*DEFINE_DEATH_TIMES_{OPTION} 
*DEFINE_DE_ACTIVE_REGION 
*DEFINE_DE_BOND 
*DEFINE_DE_BY_PART 
*DEFINE_DE_HBOND 
*DEFINE_DE_INJECTION 
*DEFINE_DE_MASSFLOW_PLANE 
*DEFINE_DE_TO_BEAM_COUPLING 
*DEFINE_DE_TO_SURFACE_COUPLING 
*DEFINE_DE_TO_SURFACE_TIED 
*DEFINE_ELEMENT_DEATH_{OPTION} 
*DEFINE_ELEMENT_GENERALIZED_SHELL 
*DEFINE_ELEMENT_GENERALIZED_SOLID 
*DEFINE_FABRIC_ASSEMBLIES 
*DEFINE_FILTER 
*DEFINE_FORMING_BLANKMESH 
*DEFINE_FORMING_CLAMP
*DEFINE_FRICTION 
*DEFINE_FRICTION_ORIENTATION 
*DEFINE_FUNCTION 
*DEFINE_FUNCTION_TABULATED 
*DEFINE_GROUND_MOTION 
*DEFINE_HAZ_PROPERTIES 
*DEFINE_HAZ_TAILOR_WELDED_BLANK 
*DEFINE_HEX_SPOTWELD_ASSEMBLY_{OPTION} 
*DEFINE_LANCE_SEED_POINT_COORDINATES 
*DEFINE_MATERIAL_HISTORIES 
*DEFINE_MULTI_DRAWBEADS_IGES 
*DEFINE_PBLAST_AIRGEO 
*DEFINE_PBLAST_GEOMETRY 
*DEFINE_PLANE 
*DEFINE_POROUS_{OPTION} 
*DEFINE_PRESSURE_TUBE 
*DEFINE_REGION 
*DEFINE_SD_ORIENTATION 
*DEFINE_SET_ADAPTIVE 
*DEFINE_SPH_ACTIVE_REGION 
*DEFINE_SPH_DE_COUPLING 
*DEFINE_SPH_INJECTION 
*DEFINE_SPH_TO_SPH_COUPLING 
*DEFINE_SPOTWELD_FAILURE_{OPTION} 
*DEFINE_SPOTWELD_FAILURE_RESULTANTS
*DEFINE_SPOTWELD_RUPTURE_PARAMETER 
*DEFINE_SPOTWELD_RUPTURE_STRESS 
*DEFINE_STAGED_CONSTRUCTION_PART 
*DEFINE_TABLE 
*DEFINE_TABLE_2D 
*DEFINE_TABLE_3D 
*DEFINE_TABLE_MATRIX 
*DEFINE_TARGET_BOUNDARY 
*DEFINE_TRACER_PARTICLES_2D 
*DEFINE_TRANSFORMATION 
*DEFINE_TRIM_SEED_POINT_COORDINATES 
*DEFINE_VECTOR 
*DEFINE_VECTOR_NODES 
Unless  noted  otherwise,  an  additional  option  “TITLE”  may  be  appended  to  the 
*DEFINE keywords.  If this option is used then an addition line is read for each section 
in 80a format which can be used to describe the defined curve, table, etc.  At present LS-
DYNA does make use of the title.  Inclusion of titles gives greater clarity to input decks. 
Examples for the *DEFINE keyword can be found at the end of this section.
*DEFINE_ADAPTIVE_SOLID_TO_DES_{OPTION} 
Purpose:    Adaptively  transform  a  Lagrangian  solid  part  or  part  set  to  DES  (Discrete 
Element  Sphere)  particles  (elements)  when  the  Lagrangian  solid  elements  comprising 
those parts fail.  One or more DES particles will be generated for each failed element as 
debris.    The  DES  particles  replacing  the  failed  element  inherit  the  properties  of  the 
failed solid element including mass, and kinematical state. 
The available options include: 
<BLANK> 
ID 
ID Card.  Additional card for the ID keyword option. 
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DID 
Type 
I 
Default 
none 
HEADING 
A70 
None 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IPID 
ITYPE 
NQ 
IPDES 
ISDES 
RSF 
OUTDES 
Type 
I 
I 
I 
I 
I 
F 
Default 
none 
none 
None 
none 
None 
1.0 
I 
0 
 VARIABLE 
DESCRIPTION
DID 
Definition ID.  This must be a unique number. 
HEADING 
Definition  descriptor.    It  is  suggested  that  unique  descriptions  be
used. 
IPID 
ID of the solid part or part set to transform.
Figure  15-1.    Left  to  right,  illustration  of  conversion  from  solid  to  DES  for
NQ = 2 of hexahedron, pentahedron, and tetrahedron elements. 
 VARIABLE 
DESCRIPTION
ITYPE 
IPID type: 
EQ.0: Part ID, 
NE.1: Part set ID. 
NQ 
Adaptive  option  for  hexahedral  elements.    For  tetrahedral  and
pentahedral elements, see Remark 1: 
EQ.1: Adapt one solid element to one discrete element, 
EQ.2: Adapt one solid element to 8 discrete elements, 
EQ.3: Adapt one solid element to 27 discrete elements. 
IPDES 
ISDES 
Part ID for newly generated discrete elements, See Remark 2. 
Section ID for discrete elements, See Remark 2. 
RSF 
DES radius scale down factor. 
OUTDES 
Allow  user  output  generated  discrete  element  nodes  and  DES
properties toa keyword file. 
EQ.0: No output.  (Default) 
EQ.1: Write data under filename, desvfill.inc 
Remarks: 
1.  DES Element to Sold Element Ratio.  The DES particles are evenly distribut-
ed within the solid element.  For hexahedral elements the number of the gener-
ated DES particles is NQ × NQ × NQ.  For pentahedral elements, the number of 
generated  DES  particles  is  1,  6,  and  18  for  NQ = 1,  2,  and  3  respectively.    For 
tetrahedral  elements,  the  number  generated  DES  particles  is  1,  4,  and  10  for 
NQ = 1, 2, and 3 respectively.  See Figure 15-1.
2.  Part ID.  The Part ID for newly generated DES particles can be either a new Part 
ID or the ID of an existing DES Part.
*DEFINE_ADAPTIVE_SOLID_TO_SPH_{OPTION} 
Purpose:    Adaptively  transform  a  Lagrangian  solid  Part  or  Part  Set  to  SPH  particles, 
when  the  Lagrangian  solid  elements  comprising  those  parts  fail.    One  or  more  SPH 
particles  (elements)  will  be  generated  for  each  failed  element.    The  SPH  particles 
replacing the failed solid Lagrangian elements inherit all the Lagrange nodal quantities 
and all the Lagrange integration point quantities of these failed solid elements.  Those 
properties  are  assigned  to  the  newly  activated  SPH  particles.    The  constitutive 
properties  assigned  to  the  new  SPH  part  will  correspond  to  the  MID  and  EOSID 
referenced by the SPH *PART definition. 
The available options include: 
<BLANK> 
ID 
ID Card.  Additional card for the ID keyword option. 
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DID 
Type 
I 
Default 
none 
HEADING 
A70 
none 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IPID 
ITYPE 
NQ 
IPSPH 
ISSPH 
ICPL 
IOPT 
CPCD 
Type 
I 
I 
I 
I 
I 
I 
I 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
average
 VARIABLE 
DESCRIPTION
DID 
Definition ID.  This must be a unique number. 
HEADING 
Definition  descriptor.    It  is  suggested  that  unique  descriptions  be
used.
VARIABLE 
DESCRIPTION
IPID 
ID of the solid part or part set to transform. 
ITYPE 
IPID type: 
EQ.0: Part ID, 
NE.0:  Part set ID. 
NQ 
Adaptive  option  for  hexahedral  elements.    For  tetrahedral  and
pentahedral elements, see remark 1: 
EQ.n: Adapt  one  8-node  solid  element  to  (𝑛 × 𝑛 × 𝑛)  SPH 
elements.  The range of n is from 1 to 8. 
IPSPH 
Part ID for newly generated SPH elements, See Remark 2. 
ISSPH 
Section ID for SPH elements, See Remark 2. 
ICPL 
Coupling  of  newly  generated  SPH  elements  to  the  adjacent  solid
elements: 
EQ.0: Failure without coupling (debris simulation), 
EQ.1: Coupled to Solid element. 
EQ.3:  Pure  thermal  coupling  between  SPH  part  and  Solid  part
(combined with IOPT = 0 option, See Remark 4). 
IOPT 
Coupling method (for ICPL = 1 only See Remark 3): 
EQ.0: Coupling  from  beginning  (used  as  constraint  between
SPH elements and Solid elements), 
EQ.1: Coupling begins when Lagrange element fails. 
CPCD 
Thermal  coupling  conductivity  between  SPH  part  and  Solid  part
for ICPL = 3 option.  The default value is set as the average value
of the conductivity from SPH part and the conductivity from Solid
part. 
Remarks: 
1.  The  SPH  particles  are  evenly  distributed  within  the  solid  element.    For 
hexahedral elements the number of the generated SPH particles is NQ*NQ*NQ.  
For pentahedral elements, the number of generated SPH particles is 1, 6, and 18 
for NQ = 1, 2, and 3 respectively.  For tetrahedral elements, the number gener-
ated SPH particles is 1, 4, and 10 for NQ = 1, 2, and 3 respectively.
2.  The  Part  ID  for  newly  generated  SPH  particles  can  be  either  a  new  Part  ID  or 
the  ID  of  an  existing  SPH  Part.    For  constraint  coupling  (i.e.    ICPL = 1  and 
IOPT = 0), the newly generated SPH part ID should be different from the exist-
ing one. 
3. 
4. 
ICPL = 0  is  used  for  debris  simulation,  no  coupling  happens  between  newly 
generated  SPH  particles  and  solid  elements,  the  user  needs  to  define  node  to 
surface contact for the interaction between those two parts.  When ICPL = 1 and 
IOPT = 1, the newly generated SPH particles are bonded with solid elements as 
one  part  through  the  coupling,  and  the  new  material  ID  with  different  failure 
criteria can be applied to the newly generated SPH particles. 
ICPL = 3 (combined with IOPT = 0) is used for pure thermal coupling between 
SPH part and Solid part only.  User can define the coupling thermal conductivi-
ty  value  between  SPH  part  and  Solid  part  through  CPCD  parameter  for  more 
realistic thermal coupling between SPH part and Solid part.
SPH node 
Example  of  SPH  nodes  for 
hexahedron 
element  with 
NQ = 2 
Example  of  SPH  nodes  for 
pentahedron  element  with 
NQ = 2 
Example  of  SPH  nodes 
tetrahedron element with NQ = 2 
for  a
Available options include: 
<BLANK> 
LOCAL 
*DEFINE_BOX 
Purpose:  Define a box-shaped volume.  Two diagonally opposite corner points of a box 
are  specified  in  global  or  local  coordinates  if  the  LOCAL  option  is  active.    The  box 
volume  is  then  used  for  various  specifications  for  a  variety  of  input  options,  e.g., 
velocities, contact, etc.  
If the option, LOCAL, is active, a local coordinate system with two vectors, see Figure 
15-7,  is  defined.    The  vector  cross  product,  𝑧 = 𝑥 × 𝑦,  determines  the  local  z-axis.    The 
local  y-axis  is  then  given  by  𝑦 = 𝑧 × 𝑥.      A  point,  X  in  the  global  coordinate  system  is 
considered  to  lie  with  the  volume  of  the  box  if  the  coordinate  X - C,  where  C  is  the 
global  coordinate  offset  vector  defined  on  Card  3,  lies  within  the  box  after  transfor-
mation into the local system, XC_local = T × ( X – C ).  The local coordinate, XC_local, is 
checked against the minimum and maximum coordinates defined on Card 1 in the local 
system.    For  the  *INCLUDE_TRANSFORM  options  that  include  translations  and 
rotations, all box options are automatically converted from *DEFINE_BOX_xxxx to *DE-
FINE_BOX_xxxx_LOCAL in the DYNA.INC file.  Here, xxxx represents the box options: 
ADAPTIVE, COARSEN, and SPH, which are defined below. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BOXID 
XMN 
XMX 
YMN 
YMX 
ZMN 
ZMX 
Type 
Default 
I 
0 
F 
F 
F 
F 
F 
F 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0
8 
*DEFINE_BOX 
Local Card 1.  First additional card for LOCAL keyword option. 
  Card 2 
Variable 
1 
XX 
Type 
F 
2 
YX 
F 
3 
ZX 
F 
4 
XV 
F 
5 
YV 
F 
6 
ZV 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Local Card 2.  Second additional card for LOCAL keyword option. 
4 
5 
6 
7 
8 
  Card 3 
Variable 
1 
CX 
Type 
F 
2 
CY 
F 
3 
CZ 
F 
Default 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
BOXID 
Box ID.  Define unique numbers. 
XMN 
XMX 
YMN 
YMX 
ZMN 
ZMX 
Minimum  x-coordinate.    Define  in  the  local  coordinate  system  if
the option LOCAL is active. 
Maximum x-coordinate.  .  Define in the local coordinate system if
the option LOCAL is active. 
Minimum y-coordinate.  .  Define in the local coordinate system if 
the option LOCAL is active. 
Maximum y-coordinate.  .  Define in the local coordinate system if
the option LOCAL is active. 
Minimum z-coordinate.  .  Define in the local coordinate system if
the option LOCAL is active. 
Maximum z-coordinate.  .  Define in the local coordinate system if
the option LOCAL is active.
XX 
YX 
ZX 
XV 
YV 
ZV 
CX 
CY 
CZ 
*DEFINE_BOX 
DESCRIPTION
X-coordinate  on  local  x-axis.    Origin  lies  at  (0,0,0).    Define  if  the 
LOCAL option is active. 
Y-coordinate  on  local  x-axis.    Define  if  the  LOCAL  option  is 
active. 
Z-coordinate  on  local  x-axis.    Define  if  the  LOCAL  option  is 
active. 
X-coordinate  of  local  x-y  vector.    Define  if  the  LOCAL  option  is 
active. 
Y-coordinate  of  local  x-y  vector.    Define  if  the  LOCAL  option  is 
active. 
Z-coordinate  of  local  x-y  vector.    Define  if  the  LOCAL  option  is 
active. 
X-global  coordinate  of  offset  vector  to  origin  of  local  system.
Define if the LOCAL option is active. 
Y-global  coordinate  of  offset  vector  to  origin  of  local  system.
Define if the LOCAL option is active. 
Z-global  coordinate  of  offset  vector  to  origin  of  local  system.
Define if the LOCAL option is active.
Available options include: 
<BLANK> 
LOCAL 
*DEFINE 
Purpose:    Define  a  box-shaped  volume  enclosing  (1)  the  shells  where  the  h-adaptive 
level (2) the solids where the tetrahedron r-adaptive mesh size is to be specified.  If the 
midpoint  of  the  element  falls  within  the  box,  the  h-adaptive  level  is  reset.    With  the 
additions  of  LIDX/NDID,  LIDY  and  LIDZ,  the  box  can  be  made  movable;  it  is  also 
possible  to  define  a  fission  box  followed  by  a  fusion  box  and  the  mesh  could  refine 
when deformed and coarsen when flattened.  Shells falling outside of this volume use 
the  value,  MAXLVL,  on  the  *CONTROL_ADAPTIVE  control  cards.    Another  related 
keyword includes: *DEFINE_CURVE_BOX_ADAPTIVITY. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BOXID 
XMN 
XMX 
YMN 
YMX 
ZMN 
ZMX 
Type 
I 
F 
F 
F 
F 
F 
F 
Default 
none 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
LEVEL 
LIDX/NDID
LIDY 
LIDZ 
BRMIN 
BRMAX 
Type 
Default 
I 
0 
I 
1 
I 
0 
I 
0 
I 
0 
F 
F 
0.0 
0.0
Local  Card  1.    First  additional  card  for  LOCAL  keyword  option.    See  *DEFINE_BOX 
for a description of the LOCAL option. 
  Card 3 
Variable 
1 
XX 
Type 
F 
2 
YX 
F 
3 
ZX 
F 
4 
XV 
F 
5 
YV 
F 
6 
ZV 
F 
7 
8 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Local Card 2.  Second additional card for LOCAL keyword option. 
4 
5 
6 
7 
8 
  Card 4 
Variable 
1 
CX 
Type 
F 
2 
CY 
F 
3 
CZ 
F 
Default 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
BOXID 
Box ID.  Define unique numbers. 
XMN 
XMX 
YMN 
YMX 
ZMN 
ZMX 
Minimum  x-coordinate.    Define  in  the  local  coordinate  system  if
the option LOCAL is active. 
Maximum x-coordinate.  Define in the local  coordinate system if
the option LOCAL is active. 
Minimum  y-coordinate.    Define  in  the  local  coordinate  system  if
the option LOCAL is active. 
Maximum y-coordinate.  Define in the local  coordinate system if
the option LOCAL is active. 
Minimum  z-coordinate.    Define  in  the  local  coordinate  system  if
the option LOCAL is active. 
Maximum  z-coordinate.    Define  in  the  local coordinate  system  if 
the option LOCAL is active.
VARIABLE   
DESCRIPTION
PID 
LEVEL 
Deformable  part  ID.    If  zero,  all  active  elements  within  box  are
considered. 
Maximum  number  of  refinement  levels  for  elements  that  are
contained in the box.  Values of 1, 2, 3, 4,...  allow a maximum of
1,  4,  16,  64,  ...    elements,  respectively,  to  be  created  for  each
original element. 
LIDX/NDID 
Load curve ID/Node ID. 
GT.0:  load  curve  ID. 
  Define  adaptive  box  movement
(displacement vs.  time) in global X axis. 
LT.0:  absolute  value  is  a  node  ID,  whose  movement  will  be
followed by the moving adaptive box.  The node ID can
be on a moving rigid body. 
EQ.0: no movement. 
LIDY 
Load curve ID. 
GT.0:  load  curve  ID. 
  Define  adaptive  box  movement
(displacement vs.  time) in global Y axis. 
EQ.0: no movement. 
LIDZ 
Load curve ID. 
GT.0:  load  curve  ID. 
  Define  adaptive  box  movement
(displacement vs.  time) in global Z axis. 
EQ.0: no movement. 
BRMIN 
Minimum mesh size in 3D tetrahedron adaptivity 
BRMAX 
Maximum mesh size in 3D tetrahedron adaptivity 
XX 
YX 
ZX 
XV 
X-coordinate  on  local  x-axis.    Origin  lies  at  (0,0,0).    Define  if  the 
LOCAL option is active. 
Y-coordinate  on  local  x-axis.    Define  if  the  LOCAL  option  is 
active. 
Z-coordinate  on  local  x-axis.    Define  if  the  LOCAL  option  is 
active. 
X-coordinate  of  local  x-y  vector.    Define  if  the  LOCAL  option  is 
active.
*DEFINE_BOX_ADAPTIVE 
DESCRIPTION
Y-coordinate  of  local  x-y  vector.    Define  if  the  LOCAL  option  is 
active. 
Z-coordinate  of  local  x-y  vector.    Define  if  the  LOCAL  option  is 
active. 
X-global  coordinate  of  offset  vector  to  origin  of  local  system.
Define if the LOCAL option is active. 
Y-global  coordinate  of  offset  vector  to  origin  of  local  system.
Define if the LOCAL option is active. 
Z-global  coordinate  of  offset  vector  to  origin  of  local  system. 
Define if the LOCAL option is active. 
YV 
ZV 
CX 
CY 
CZ 
Remarks: 
The  moving  adaptive  box  is  very  useful  and  efficient  in  situation  where  deformation 
progresses  while  happening  only  locally,  such  as  roller  hemming  and  incremental 
forming  simulation.    With  the  moving  box  feature,  elements  entering  one  box  can  be 
refined  and  fused  together  when  they  enter  another  box.    Mesh  fission  outside  of  the 
moving  box  envelope  is  controlled  by  MAXLVL  and  other  parameters  under 
*CONTROL_ADAPTIVE.    The  fusion  controls  (NCFREQ,  IADPCL)  can  be  defined 
using *CONTROL_ADAPTIVE.  Currently, only IADPCL = 1 is supported. 
Only  when  one  of  the  LCIDX/NDID,  LICDY,  or  LCIDZ  is  defined,  the  adaptive  box 
will be moving; otherwise it will be stationary. 
For 3D tetrahedron r-adaptivity, the current implementation does not support LOCAL 
option.    In  card  2,  PID,  BRMIN  and  BRMAX  are  the  only  parameters  currently 
supported in 3D r-adaptivity. 
Example: 
Referring to a partial input deck below, and Figure 15-2, a strip of sheet metal is being 
roller  hemmed.    The  process  consists  of  pre-  and  final  hemming.    Each  pre-  and  final 
roller  is  defined  with  a  moving  adaptive  box  ID  2  and  3,  respectively,  with  the  box 
shapes shown in Figure 15-2.  The first box, a fission box, was set at LEVEL = 3, while 
the  second  box,  a  fusion  box,  was  set  at  LEVEL = 1.    Elements  outside  of  the  volume 
envelope  made  by  the  moving  boxes  undergo  no  fission  and  fusion  (MAXLVL = 1).  
This settings allows mesh fission when entering the moving box 2 (LEVEL = 3), fusion 
only  when  elements  entering  the  moving  box  3  (LEVEL = 1),  no  fusion/fusion 
(MAXLVL = 1) at all outside of the volume envelope created by the moving boxes.  In
the example, the boxes 2 and 3 are to be moved in global X direction for a distance of 
398mm defined by load curve 11, and 450mm defined by load curve 12, respectively. 
*CONTROL_TERMINATION 
0.252 
*CONTROL_ADAPTIVE 
$  ADPFREQ    ADPTOL    ADPOPT    MAXLVL    TBIRTH    TDEATH     LCADP    IOFLAG 
   8.05E-4  0.200000         2         1     0.0001.0000E+20         0         1 
$  ADPSIZE    ADPASS    IREFLG    ADPENE     ADPTH    MEMORY    ORIENT     MAXEL 
  0.300000         1         0       5.0 
$  IADPN90              NCFREQ    IADPCL    ADPCTL    CBIRTH    CDEATH 
        -1         0         1         1      10.0     0.000      10.30 
*DEFINE_BOX_ADAPTIVE 
$#   BOXID       XMN       XMX       YMN       YMX       ZMN       ZMX 
         2 -10.00000 36.000000 -15.03000  3.991000  1.00E+00 48.758000 
$#     PID     LEVEL LIDX/NDID      LIDY      LIDZ 
         6         3        11 
*DEFINE_BOX_ADAPTIVE 
$#   BOXID       XMN       XMX       YMN       YMX       ZMN       ZMX 
         3 -100.0000  -60.0000 -15.03000  3.991000  1.00E+00 48.758000 
$#     PID     LEVEL LIDX/NDID      LIDY      LIDZ 
         6         1        12 
*DEFINE_CURVE 
11 
               0.000                 0.0 
          0.00100000                 1.0 
          0.19900000               397.0 
          0.20000000               398.0 
               1.000               398.0 
      ⋮ 
      ⋮  
*DEFINE_CURVE 
12 
                 0.0                 0.0 
                0.05                 0.0 
               0.051                 1.0 
               0.251               401.0 
               0.252               450.0 
      ⋮ 
      ⋮  
A moving box can also follow the movement of a node, which can be on a moving rigid 
body.  In this case, load curves defining the boxes’ movement can be skipped, instead, 
NDIDs  for  the  boxes  should  be  defined.    For  example,  in  Figure  15-2  and  a  partial 
keyword example below, box 2 is to follow a node (ID: 33865) on the pre-roller, and box 
3 to follow another node (ID: 38265) on the final roller. 
*DEFINE_BOX_ADAPTIVE 
$#   BOXID       XMN       XMX       YMN       YMX       ZMN       ZMX 
         2 -10.00000 36.000000 -15.03000  3.991000  1.00E+00 48.758000 
$#     PID     LEVEL LIDX/NDID      LIDY      LID 
         6         3    -33865 
*DEFINE_BOX_ADAPTIVE 
$#   BOXID       XMN       XMX       YMN       YMX       ZMN       ZMX 
         3 -100.0000  -60.0000 -15.03000  3.991000  1.00E+00 48.758000 
$#     PID     LEVEL LIDX/NDID      LIDY      LID 
         6         3    -38265
*DEFINE_BOX_ADAPTIVE 
The variables LIDX/NDID, LIDY, LIDZ are available in both SMP and MPP starting in 
Revision 98718.
Fission box: LEVEL=3,
follows Node 38265 
Node 33865
Inner part
Outer flange
Hem bed
Roller path
Pre-roller
Node 38265
Final roller
Fusion box 3: LEVEL=1, 
follows Node 33865
Hem bed
Mesh fissioned after 
pre-rollers' passing
Mesh fuzed after all 
rollers' passing
Inner part
Original mesh
Roller path
Outer flange
Figure 15-2.  Defining mesh fission and fusion.
*DEFINE_BOX_COARSEN_{OPTION} 
Available options include: 
<BLANK> 
LOCAL 
Purpose:  Define a specific box-shaped volume indicating elements which are protected 
from mesh coarsening.  See also *CONTROL_COARSEN. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BOXID 
XMN 
XMX 
YMN 
YMX 
ZMN 
ZMX 
IFLAG 
Type 
I 
F 
F 
F 
F 
F 
F 
Default 
none 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
I 
0 
Local  Card  1.    First  additional  card  for  LOCAL  keyword  option.    See  *DEFINE_BOX 
for a description of the LOCAL option. 
  Card 2 
Variable 
1 
XX 
Type 
F 
2 
YX 
F 
3 
ZX 
F 
4 
XV 
F 
5 
YV 
F 
6 
ZV 
F 
7 
8 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Local Card 2.  Second additional card for LOCAL keyword option. 
4 
5 
6 
7 
8 
  Card 3 
Variable 
1 
CX 
Type 
F 
2 
CY 
F 
3 
CZ 
F 
Default 
0.0 
0.0 
0.0
VARIABLE   
DESCRIPTION
BOXID 
Box ID.  Define unique numbers. 
XMN 
XMX 
YMN 
YMX 
ZMN 
ZMX 
Minimum  x-coordinate.    Define  in  the  local  coordinate  system  if
the option LOCAL is active. 
Maximum x-coordinate.  .  Define in the local coordinate system if
the option LOCAL is active. 
Minimum y-coordinate.  .  Define in the local coordinate system if
the option LOCAL is active. 
Maximum y-coordinate.  .  Define in the local coordinate system if 
the option LOCAL is active. 
Minimum z-coordinate.  .  Define in the local coordinate system if
the option LOCAL is active. 
Maximum z-coordinate.  .  Define in the local coordinate system if
the option LOCAL is active. 
IFLAG 
Flag for protecting elements inside or outside of box. 
EQ.0: elements inside the box cannot be coarsened 
EQ.1: elements outside the box cannot be coarsened 
XX 
YX 
ZX 
XV 
YV 
ZV 
CX 
X-coordinate  on  local  x-axis.    Origin  lies  at  (0,0,0).    Define  if  the 
LOCAL option is active. 
Y-coordinate  on  local  x-axis.    Define  if  the  LOCAL  option  is 
active. 
Z-coordinate  on  local  x-axis.    Define  if  the  LOCAL  option  is 
active. 
X-coordinate  of  local  x-y  vector.    Define  if  the  LOCAL  option  is 
active. 
Y-coordinate  of  local  x-y  vector.    Define  if  the  LOCAL  option  is 
active. 
Z-coordinate  of  local  x-y  vector.    Define  if  the  LOCAL  option  is 
active. 
X-global  coordinate  of  offset  vector  to  origin  of  local  system.
Define if the LOCAL option is active.
Y-global  coordinate  of  offset  vector  to  origin  of  local  system.
Define if the LOCAL option is active. 
Z-global  coordinate  of  offset  vector  to  origin  of  local  system.
Define if the LOCAL option is active. 
*DEFINE 
  VARIABLE   
CY 
CZ 
Remarks: 
1.  Many boxes may be defined.  If an element is protected by any box then it may 
not be coarsened.
*DEFINE 
Purpose:  Define a specific box or tube shaped volume around a draw bead.  This option 
is  useful  for  the  draw  bead  contact.    If  box  shaped,  the  volume  will  contain  the  draw 
bead nodes and elements between the bead and the outer edge of the blank.  If tubular, 
the tube is centered around the draw bead.  All elements within the tubular volume are 
included in the contact definition.  
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BOXID 
PID 
SID 
IDIR 
STYPE 
RADIUS 
CID 
Type 
Default 
I 
0 
F 
F 
F 
0.0 
0.0 
0.0 
I 
4 
F 
0.0 
I 
0 
Remarks 
optional  optional 
  VARIABLE   
DESCRIPTION
BOXID 
Box ID.  Define unique numbers. 
PID 
SID 
IDIR 
Part ID of blank. 
Set ID that defines the nodal points that lie along the draw bead.
If a node set is defined, the nodes in the set must be consecutive
along the draw bead.  If a part or part set is defined, the set must
consist  of  beam  or  truss  elements.    Within  the  part  set,  no 
ordering  of  the  elements  is  assumed,  but  the  number  of  nodes
must equal the number of beam elements plus 1. 
Direction  of  tooling  movement.      The  movement  is  in  the  global
coordinate  direction  unless  the  tubular  box  option  is  active  and
CID  is  nonzero.    In  this  latter  case,  the  movement  is  in  the  local
coordinate direction. 
EQ.1: tooling moves in x-direction, 
EQ.2: tooling moves in y-direction, 
EQ.3: tooling moves in z-direction.
STYPE 
Set type: 
*DEFINE_BOX_DRAWBEAD 
DESCRIPTION
EQ.2: part set ID, 
EQ.3: part ID, 
EQ.4: node set ID. 
RADIUS 
The radius of the tube, which is centered around the draw bead.
Elements of part ID, PID, that lie within the tube will be included
in the contact.    If the radius is not defined, a rectangular box is
used  instead.    This  option  is  recommended  for  curved  draw 
beads  and  for  draw  beads  that  are  not  aligned  with  the  global
axes. 
CID 
Optional coordinate system ID.  This option is only available for
the tubular drawbead.
Available options include: 
<BLANK> 
LOCAL 
*DEFINE 
Purpose:  Define a box-shaped volume.  Two diagonally opposite corner points of a box 
are  specified  in  global  coordinates.    Particle  approximations  of  SPH  elements  are 
computed  when  particles  are  located  inside  the  box.    The  load  curve  describes  the 
motion of the maximum and minimum coordinates of the box. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BOXID 
XMN 
XMX 
YMN 
YMX 
ZMN 
ZMX 
VID 
Type 
I 
F 
F 
F 
F 
F 
F 
Default 
none 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
4 
5 
6 
7 
  Card 2 
1 
Variable 
LCID 
Type 
Default 
I 
0 
2 
VD 
I 
0 
3 
NID 
I 
0 
I 
0
Local  Card  1.    First  additional  card  for  LOCAL  keyword  option.    See  *DEFINE_BOX 
for a description of the LOCAL option 
  Card 3 
Variable 
1 
XX 
Type 
F 
2 
YX 
F 
3 
ZX 
F 
4 
XV 
F 
5 
YV 
F 
6 
ZV 
F 
7 
8 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Local Card 2.  Second additional card for LOCAL keyword option. 
4 
5 
6 
7 
8 
  Card 4 
Variable 
1 
CX 
Type 
F 
2 
CY 
F 
3 
CZ 
F 
Default 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
BOXID 
Box ID.  Define unique numbers. 
XMN 
XMX 
YMN 
YMX 
ZMN 
ZMX 
Minimum  x-coordinate.    Define  in  the  local  coordinate  system  if
the option LOCAL is active. 
Maximum x-coordinate.  Define in the local  coordinate system if
the option LOCAL is active. 
Minimum  y-coordinate.    Define  in  the  local  coordinate  system  if
the option LOCAL is active. 
Maximum y-coordinate.  Define in the local  coordinate system if
the option LOCAL is active. 
Minimum  z-coordinate.    Define  in  the  local  coordinate  system  if 
the option LOCAL is active. 
Maximum  z-coordinate.    Define  in  the  local coordinate  system  if
the option LOCAL is active.
VARIABLE   
DESCRIPTION
VID 
LCID 
Vector ID for DOF, see *DEFINE_VECTOR. 
Load  curve  ID  to  describe  motion  value  versus  time,  see  *DE-
FINE_CURVE 
VD 
Velocity/Displacement flag: 
EQ.0: velocity, 
EQ.1: displacement, 
EQ.2: referential node 
NID 
Referential  nodal  ID  for  VD = 2  (SPH  box  will  move  with  this 
node). 
XX 
YX 
ZX 
XV 
YV 
ZV 
CX 
CY 
CZ 
X-coordinate  on  local  x-axis.    Origin  lies  at  (0,0,0).    Define  if  the 
LOCAL option is active. 
Y-coordinate  on  local  x-axis.    Define  if  the  LOCAL  option  is 
active. 
Z-coordinate  on  local  x-axis.    Define  if  the  LOCAL  option  is 
active. 
X-coordinate  of  local  x-y  vector.    Define  if  the  LOCAL  option  is 
active. 
Y-coordinate  of  local  x-y  vector.    Define  if  the  LOCAL  option  is 
active. 
Z-coordinate  of  local  x-y  vector.    Define  if  the  LOCAL  option  is 
active. 
X-global  coordinate  of  offset  vector  to  origin  of  local  system.
Define if the LOCAL option is active. 
Y-global  coordinate  of  offset  vector  to  origin  of  local  system.
Define if the LOCAL option is active. 
Z-global  coordinate  of  offset  vector  to  origin  of  local  system.
Define if the LOCAL option is active.
*DEFINE_CONNECTION_PROPERTIES_{OPTION} 
Available options include: 
<BLANK> 
ADD 
Purpose:    Define  failure  related  parameters  for  solid  element  spot  weld  failure  by 
*MAT_SPOTWELD_DAIMLERCHRYSLER.  For each connection identifier, CON_ID, a 
separate *DEFINE_CONNECTION_PROPERTIES section must be included.  The ADD 
option allows material specific properties to be added to an existing connection ID.  See 
Remark 2. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CON_ID 
PRUL 
AREAEQ 
DGTYP  MOARFL 
Type 
Default 
F 
0 
  Card 2 
1 
I 
0 
2 
I 
0 
3 
4 
I 
0 
5 
I 
0 
6 
7 
8 
Variable 
DSIGY 
DETAN 
DDGPR 
DRANK 
DSN 
DSB 
DSS 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
1010 
none 
none 
none 
none
Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DEXSN 
DEXSB 
DEXSS 
DLCSN 
DLCSB 
DLCSS 
DGFAD  DSCLMRR
Type 
F 
F 
F 
Default 
1.0 
1.0 
1.0 
I 
0 
I 
0 
I 
0 
F 
F 
none 
1.0 
Material Specific Data: 
For each shell material with material specific data, define for this CON_ID the following 
two  cards.    Add  as  many  pairs  of  cards  as  necessary.    This  input  is  terminated  by  the 
next keyword (“*”) card. 
Material Data Card 1. 
  Card 4 
1 
2 
3 
4 
5 
Variable 
MID 
SGIY 
ETAN 
DGPR 
RANK 
Type 
F 
F 
F 
F 
F 
Default 
1010 
6 
SN 
F 
7 
SB 
F 
8 
SS 
F 
Material Data Card 2. 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EXSN 
EXSB 
EXSS 
LCSN 
LCSB 
LCSS 
GFAD 
SCLMRR 
Type 
F 
F 
F 
I 
I 
I 
F 
F 
Default 
  VARIABLE   
CON_ID 
1.0 
DESCRIPTION
Connection  ID,  referenced  on  *MAT_SPOTWELD_DAIMLER-
CHRYSLER.    Multiple  sets  of  connection  data  may  be  used  by
assigning different connection IDs.
*DEFINE_CONNECTION_PROPERTIES 
DESCRIPTION
PRUL 
The failure rule number for this connection. 
EQ.1:  Use data of weld partner with lower RANK (default). 
GE.2:  Use  DEFINE_FUNCTION  expressions  to  determine 
weld  data  depending  on  several  values  of  both  weld
partners.    Variables  DSIGY,  DETAN,  DDGPR,  DSN, 
DSB, DSS, DEXSN, DEXSB, DEXSS, and DGFAD must be 
defined as function IDs, see Remark 5. 
AREAEQ 
Area equation number for the connection area calculation. 
EQ.0:  (default) Areatrue = Areamodelled 
EQ.1:  millimeter form; see Remark 4 
EQ.-1:  meter form; see Remark 4 
DGTYP 
Damage type 
EQ.0: 
EQ.1: 
EQ.2: 
no damage function is used 
strain based damage 
failure function based damage 
EQ.3 or 4:  fading energy based damage; see Remark 4 
MOARFL 
Modeled area flag 
EQ.0: Areamodelled goes down with shear (default) 
EQ.1: Areamodelled stays constant 
DSIGY 
Default yield stress for the spot weld element. 
DETAN 
Default tangent modulus for the spot weld element. 
DDGPR 
Default damage parameter for hyperbolic based damage function.
DRANK 
Default rank value. 
DSN 
DSB 
DSS 
Default normal strength. 
Default bending strength. 
Default shear strength. 
DEXSN 
Default exponent on normal stress term. 
DEXSB 
Default exponent on bending stress term.
VARIABLE   
DESCRIPTION
DEXSS 
Default exponent on shear stress term. 
DLCSN 
DLCSB 
DLCSS 
Default curve ID for normal strength scale factor as a function of
strain rate. 
Default curve ID for bending strength scale factor as a function of
strain rate. 
Default  curve  ID  for  shear  strength  scale  factor  as  a  function  of
strain rate. 
DGFAD 
Default fading energy for damage type 3 and type 4. 
DSCLMRR 
Default scaling factor for torsional moment in failure function. 
MID 
SIGY 
ETAN 
DGPR 
Material ID of the shell material for which properties are defined.
Yield stress to be used in the spot weld element calculation. 
Tangent modulus to be used in the spot weld element calculation.
Damage parameter for hyperbolic based damage function. 
RANK 
Rank value.  See Remark 4. 
SN 
SB 
SS 
EXSN 
EXSB 
EXSS 
LCSN 
LCSB 
LCSS 
Normal strength. 
Bending strength. 
Shear strength. 
Exponent on normal stress term. 
Exponent on bending stress term. 
Exponent on shear stress term. 
Curve  ID  for  normal  strength  scale  factor  as  a  function  of  strain
rate. 
Curve ID for bending strength scale factor as a function of strain 
rate. 
Curve  ID  for  shear  strength  scale  factor  as  a  function  of  strain
rate.
*DEFINE_CONNECTION_PROPERTIES 
DESCRIPTION
GFAD 
Fading energy for damage type 3 and 4. 
SCLMRR 
Scaling factor for torsional moment in failure function. 
Remarks: 
1.  Restriction  to  *MAT_SPOTWELD_DAIMLERCHHRYSLER.    This  keyword  is 
used  only  with  *MAT_SPOTWELD_DAIMLERCHRYSLER.    The  data  input  is 
used  in  a  3  parameter  failure  model.    Each  solid  spot  weld  element  connects 
shell elements that may have the same or different materials.  The failure model 
assumes that failure of the spot weld depends on the properties of the welded 
materials, so this keyword allows shell material specific data to be input for the 
connection.  The default data will be used for any spot weld connected to a shell 
material that does not have material specific data defined, so it is not necessary 
to define material specific data for all welded shell materials. 
2.  ADD Option.  To simplify data input, the ADD keyword option allows material 
specific  data  to  be  added  to  an  existing  *DEFINE_CONNECTION_PROPER-
TIES table.   To use the ADD option, omit cards 2 and 3, and input only CON_-
ID on card 1.  Then use cards 4 and 5 to input material specific data.  For each 
unique  CON_ID,  control  parameters  and  default  values  must  be  input  in  one 
set  of  *DEFINE_CONNECTION_PROPERTIES  data.    The  same  CON_ID  may 
be  used  for  any  number  of  sets  of  material  specific  data  input  with  the  ADD 
option.   
3.  The Three Parameter Failure Function.  The three parameter failure function 
is 
𝐹)
𝑓 = (
𝜎𝑛
𝜎𝑛
𝑚𝑏
  + (
𝑚𝑛
  + (
𝜎𝑏
𝜎𝑏
where the three strength terms are SN, SB, and SS, and the three exponents are 
EXSN, EXSB, and EXSS.  The strengths may be a function of strain rate by using 
the load curves, LCSN, LCSB, and LCSS.  The peak stresses in the numerators 
are calculated from force resultants and simple beam theory. 
𝜏𝐹)
𝑚𝜏
  − 1 , 
𝐹)
𝜎𝑛 =
𝑁𝑟𝑟
,
𝜎𝑏 =
2 + 𝑀𝑟𝑡
√𝑀𝑟𝑠
,
𝜏 = SCLMRR ×
𝑀𝑟𝑟
2𝑍
+
2 + 𝑁𝑟𝑡
√𝑁𝑟𝑠
where the area is the cross section area of the weld element and Z is given by: 
𝑍 = 𝜋
𝑑3
32
where d  is  the  equivalent  diameter  of  the  solid  spot  weld  element  assuming  a 
circular cross section.
4.  Control  Parameters  PRUL,  AREAQ.    And  DGTYP.    There  are  three  control 
parameters  that  define  how  the  table  data  will  be  used  for  the  connection, 
PRUL,  AREAEQ,  and  DGTYP.    PRUL  determines  how  the  parameters  will  be 
used.    Because  each  weld  connects  two  shell  surfaces,  one  weld  can  have  two 
sets  of  failure  data  as  well  as  two  values  for  ETAN  and  SIGY.    For  PRUL=1 
(default), a simple rule is implemented and the data with the lower RANK will 
be used.  For PRUL=2 or 3, function expressions can be used to determine the 
data based on several input values from both weld partners . 
The second control parameter is AREAEQ which specifies a rule for calculating 
a true weld cross section area, 𝐴true to be used in the failure function in place of 
the modeled solid element area, 𝐴.  For AREAEQ = 1, 𝐴true is calculated by 
(5√𝑡min shell)
𝐴true =
where 𝑡min shell is the thickness of the welded shell  surface that has the  smaller 
thickness.  For AREAEQ = −1, 𝐴true is calculated by 
𝐴true =
(
1000
√1000 × 𝑡min shell)
The equation for AREAEQ = 1 is valid only for a length unit of millimeters, and 
AREAEQ = −1 is valid only for a length unit of meters. 
The  third  control  parameter,  DGTYP,  chooses  from  two  available  damage 
types.    For  DGTYP = 0,  damage  is  turned  off  and  the  weld  fails  immediately 
when 𝑓 ≥ 0. For DGTYP > 0, damage is initiated when 𝑓 ≥ 0 and complete fail-
ure occurs when 𝜔 ≥ 1.  For DGTYP = 1, damage growth is a function of plastic 
strain: 
𝜔 =
𝑝 − 𝜀failure
𝜀eff
− 𝜀failure
𝜀rupture
,
𝜀failure
≤ 𝜀eff
𝑝 ≤ 𝜀rupture
𝑝  is the effective plastic strain in the weld material.  When the value of 
where 𝜀eff
the failure function first exceeds zero, the plastic strain at failure𝜀failure
 is set to 
the current plastic strain, and the rupture strain is offset from the plastic strain 
at failure by   
𝜀rupture
= 𝜀failure
+  RS − EFAIL 
where  RS  and  EFAIL  are  the  rupture  strain  and  plastic  strain  at  failure  which 
are  input  on  the  *MAT_SPOTWELD_DAIMLERCHRYSLER  card.    If  failure 
occurs when the plastic strain is zero, the weld material yield stress is reduced 
to the current effective stress such that damage can progress. 
For DGTYP = 2, damage is a function of the failure function, f:
𝑓 ≥ 0 ⇒ 𝜔 =
𝑓rupture
where 𝑓rupture is the value of the failure function at rupture which is defined by 
𝑓rupture = RS − EFAIL 
and RS and EFAIL are input on the *MAT_SPOTWELD_DAIMLERCHRYSLER 
card. 
Because the DGTYP = 1 damage function is scaled by plastic strain, it will mon-
otonically increase in time.  The DGTYP = 2  damage function is  forced to be a 
monotonically increasing function in time by using the maximum of the current 
value and the maximum previous value.  For both DGTYP = 1 and DGTYP = 2, 
the stress scale factor is then calculated by 
𝜎̂ =
DGPR × (1 − 𝜔)
𝜎 
𝜔 (1
+ √1
+ DGPR) + DGPR
This equation becomes nearly linear at the default value of DGPR which is 1010. 
For DGTYP = 3, damage is a function of total strain: 
𝜔 =
∆𝜀𝑛
∆𝜀fading
where Δ𝜀𝑛 is the accumulated total strain increment between moment of dam-
age initiation (failure) and current time step 𝑡𝑛  
∆𝜀𝑛 = ∆𝜀𝑛−1 + ∆𝑡𝑛√
 tr(𝛆̇𝑛𝜺̇𝑛
T) ,
∆𝜀|𝑡failure = 0 
and 𝛥𝜀𝑓𝑎𝑑𝑖𝑛𝑔 is the total strain increment for fading (reduction of stresses to zero)  
∆𝜀fading =
2 × GFAD
𝜎failure
where GFAD is the fading energy from input and 𝜎failure is the effective stress at 
failure.  The stress scale factor is then calculated by a linear equation 
𝜎̂ = (1 − 𝜔)𝜎 
where 𝜎 is the Cauchy stress tensor at failure and 𝜔 is the actual damage value.  
Problems  can  occur,  if  the  loading  direction  changes  after  the  onset  of  failure, 
since during the damage process, the components of the stress tensor are kept 
constant and hence represent the stress state at failure. 
Therefore  DGTYP = 4  should  be  used  describing  the  damage  behavior  of  the 
spotweld in a more realistic way.  For DGTYP = 4, damage is a function of the 
internal work done by the spotweld after failure,
𝜎̂ = (1 − 𝜔)𝜎 ep, 𝜔 =  
𝐺used
2 × GFAD 
, 𝐺used = 𝐺used
𝑛−1 + det (𝐹𝑖𝑗𝜎𝑖𝑗
epΔ𝜀𝑖𝑗) 
Therein,  𝐹𝑖𝑗  is  the  deformation  gradient.  𝜎 ep  is  a  scaled  Cauchy  stress  tensor 
based  on  the  undamaged  Cauchy  stress  tensor  𝜎 wd  and  scaled  in  such  a  way 
that the same internal work is done in the current time step as in the time step 
before (equipotential): 
𝜎 ep = 𝛼𝜎 wd, 𝛼 =  
𝑛−1,epΔ𝜀𝑖𝑗
𝜎𝑖𝑗
wdΔ𝜀𝑖𝑗
𝜎𝑖𝑗
5.  Failure Rule from *DEFINE_FUNCTION.  The failure rule number PRUL = 2 or 
3,  is  available  starting  with  Release  R7.    To  use  this  new  option,  11  variables 
have to be defined as function IDs: DSIGY, DETAN, DDGPR, DSN, DSB, DSS, 
DEXSN, DEXSB, DEXSS,  DGFAD, and DSCLMRR. 
These functions depend on: 
(t1, t2) = thicknesses of both weld partners 
(sy1, sy2) = initial yield stresses at plastic strain 
(sm1, sm2) = maximum engineering yield stresses 
𝑟 = strain rate 
𝑎 = spot weld area 
For DSIGY = 100 Such a function could look like: 
*DEFINE_FUNCTION 
        100 
 func(t1,t2,sy1,sy2,sm1,sm2,r,a)=0.5*(sy1+sy2) 
All the listed arguments in their correct order must be included in the argument 
list.  For PRUL = 2, the thinner part is the first weld partner.  For PRUL = 3, the 
bottom part (nodes 1-2-3-4) is the first weld partner.  Since material parameters 
have to be identified from both weld partners during initialization, this feature 
is only available for a subset of material models at the moment, namely material 
types 24, 120, 123, and 124.  This new option eliminates the need for the ADD 
option.
*DEFINE_CONSTRUCTION_STAGES 
Purpose:  Define times and durations of construction stages. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ISTAGE 
ATS 
ATE 
ATR 
RTS 
RTE 
Type 
I 
F 
F 
F 
F 
F 
Default 
none 
0.0 
0.0 
none 
ATS 
ATE 
  VARIABLE   
DESCRIPTION
ISTAGE 
Stage ID 
Analysis time at start of stage 
Analysis time at end of stage 
Analysis time duration of ramp 
Real time at start of stage 
Real time at end of stage 
ATS 
ATE 
ATR 
RTS 
RTE 
Remarks: 
See  also  *CONTROL_CONSTRUCTION_STAGES  and  *DEFINE_STAGED_CON-
STRUCTION_PART.  
The  first  stage  should  start  at  time  zero.    There  must  be  no  gaps  between  stages,  i.e.  
ATS for each stage must be the same as ATE for the previous stage. 
The  ramp  time  allows  gravity  loading  and  part  stiffening/removal  to  be  applied 
gradually during the first time period ATR of the construction stage. 
The analysis always runs in “analysis time” – typically measured in seconds.  The “real 
time” is used only as a number to appear on output plots and graphs, and is completely 
arbitrary.  A dynain file is written at the end of each stage.
*DEFINE 
Purpose:    Exclude  tied  nodes  from  being  treated  in  specific  contact  interfaces.    This 
keyword is currently only available in the MPP version. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EID 
Type 
I 
Title 
A70 
ID Card 1.  This card sets the contact interface the ids of up to 7 tied interfaces. 
  Card 2 
1 
Variable 
Target 
Type 
I 
2 
C1 
I 
3 
C2 
I 
4 
C3 
I 
5 
C4 
I 
6 
C5 
I 
7 
C6 
I 
8 
C7 
I 
Optional ID Cards.  More tied interfaces.  Include as many cards as necessary. 
  Card 2 
Variable 
1 
C8 
Type 
I 
2 
C9 
I 
3 
4 
5 
6 
7 
8 
C10 
C11 
C12 
C13 
C14 
C15 
I 
I 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
EID 
Title 
Target 
Exclusion ID 
Exclusion Title 
Contact interface from which tied nodes are to be excluded.  This
must  be  the  ID  of  a  SINGLE_SURFACE,  NODE_TO_SURFACE, 
or SURFACE_TO_SURFACE contact with SOFT ≠ 2.
Ci 
*DEFINE_CONTACT_EXCLUSION 
DESCRIPTION
The IDs of TIED contacts: 7 on the first card and 8 per additional
card for as many cards as necessary. 
Any node which is a slave node in one of these interfaces, and is
in  fact  tied,  will  not  be  processed  (as  a  slave  node)  in  the  Target
interface. 
Note  that  if  a  node  is  excluded  from  the  Target  by  this
mechanism, contact forces may still be applied to the node due to 
any  slave  or  master  nodes  impacting  the  contact  segments  of
which it is a part (no contact SEGMENTS are deleted, only contact
NODES). 
If the Target contact is of type SURFACE_TO_SURFACE, any tied 
slave  nodes  are  deleted  from  both  the  slave  side  (for  the  normal
treatment) and the master side (for the symmetric treatment).
*DEFINE 
Purpose:  Define a rectangular, a cylindrical, or a spherical volume in a local coordinate 
system.  The volume can be referenced by *SET_NODE_GENERAL for the purpose of 
defining a node set consisting of nodes inside the volume, or by *CONTACT_...  for the 
purpose  of  defining  nodes  or  segments  on  the  slave  side  or  the  master  side  of  the 
contact . 
  Card 1 
1 
2 
3 
Variable 
CVID 
CID 
TYPE 
Type 
Default 
I 
0 
I 
0 
I 
0 
4 
XC 
F 
0. 
5 
YC 
F 
0. 
6 
ZC 
F 
0. 
7 
8 
Card 2 for Rectangular Prism.  Use when type = 0. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
XMN 
XMX 
YMN 
YMX 
ZMN 
ZMX 
Type 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Card 2 for Cylinder.  Use when type = 1. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LENGTH 
RINNER 
ROUTER  D_ANGC 
Type 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0
Card 2 for Sphere  Use when type = 3. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RINNER 
ROUTER  D_ANGS 
Type 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
CVID 
CID 
TYPE 
XC 
YC 
ZC 
XMN 
XMX 
YMN 
YMX 
ZMN 
ZMX 
Contact volume ID 
Coordinate  system  ID.    Required  for  rectangular  and  cylindrical
volumes 
Volume type.  Set to 0 for rectangular, 1 for cylindrical, and 2 for
spherical. 
x-coordinate which defines the origin of coordinate system or the
center  of  the  sphere  for  type = 3  referenced  to  the  global 
coordinate system. 
y-coordinate which defines the origin of coordinate system or the
center  of  the  sphere  for  type = 3  referenced  to  the  global 
coordinate system. 
z-coordinate which defines the origin of coordinate system or the 
center  of  the  sphere  for  type = 3  referenced  to  the  global 
coordinate system. 
Minimum x-coordinate in local coordinate system. 
Maximum x-coordinate in local coordinate system. 
Minimum y-coordinate in local coordinate system. 
Maximum y-coordinate in local coordinate system. 
Minimum z-coordinate in local coordinate system. 
Maximum z-coordinate in local coordinate system.
VARIABLE   
LENGTH 
DESCRIPTION
Length  of  cylinder  originating  at  (XC,YC,ZC)  and  revolving
around the local x-axis. 
RINNER 
Inner radius of cylinder or sphere. 
ROUTER 
Outer radius of cylinder or sphere. 
D_ANGC 
D_ANGS 
If  the  included  angle  between  the  axis  of  the  cylinder  and  the
normal  vector  to  the  contact  segment  is  less  than  this  angle,  the 
segment is deleted.   
If  the  included  angle between a  line  draw  from  the  center  of the
sphere  to  the  centroid  of  the  segment,  and  the  normal  vector  to
the  contact  segment  is  greater  than  this  angle,  the  segment  is 
deleted.
*DEFINE_COORDINATE_NODES 
Purpose:    Define  a  local  coordinate  system  with  three  node  numbers.    The  local 
cartesian coordinate system is defined in the following steps.  If the primary direction is 
along  the  x-axis,  then  the  𝑧-axis  is  computed  from  the  cross  product  of  𝑥  and  𝑦̅,  ,  𝑧 = 𝑥 × 𝑦̅,  then  the  𝑦-axis  is  computed  via  𝑦 = 𝑧 × 𝑥.    A  similar  procedure 
applies if the local axis is along the y or z axes.   
Card 
1 
Variable 
CID 
Type 
Default 
I 
0 
2 
N1 
I 
0 
3 
N2 
I 
0 
4 
N3 
I 
0 
5 
6 
7 
8 
FLAG 
DIR 
I 
0 
A 
X 
  VARIABLE   
DESCRIPTION
CID 
Coordinate system ID.  A unique number has to be defined. 
N1 
N2 
N3 
FLAG 
ID of node located at local origin. 
ID  of  node  located  along  local  x-axis  if  DIR = X,  the  y-axis  if 
DIR = Y, and along the z axis if DIR = Z. 
ID of node located in local x-y plane if DIR = X, the local y-z plane 
if DIR = Y, and the local z-x plane if DIR = Z. 
Set to unity, 1, if the local system is to be updated each time step.
Generally,  this  option  when  used  with  nodal  SPC's  is  not 
recommended  since  it  can  cause  excursions  in  the  energy  balance 
because  the  constraint  forces  at  the  node  may  go  through  a
displacement if the node is partially constrained. 
DIR 
Axis defined by node  N2 moving from the origin node N1.  The
default direction is the x-axis. 
Remarks: 
1.  The nodes N1, N2, and N3 must be separated by a reasonable distance and not 
colinear to avoid numerical inaccuracies.
Figure 15-3.  Definition of local coordinate system using three nodes when the
node N2 lies along the x-axis.
*DEFINE_COORDINATE_SYSTEM_{OPTION} 
Available options include: 
<BLANK> 
IGES 
Purpose:  Define a local coordinate system.   
This  card  implements  the  same  method  as  *DEFINE_COORDINATE_NODES;  but, 
instead  of  reading  coordinate  positions  from  nodal  IDs,  it  directly  reads  the  three 
coordinates from its data cards as Cartesian triples. 
When the IGES option is active, LS-DYNA will generate the coordinate system from an 
IGES file containing three straight curves representing the x, y, and z axes.  See remark 
4. 
Card 1 for <BLANK> Keyword Option. 
  Card 1 
1 
Variable 
CID 
Type 
Default 
I 
0 
2 
XO 
F 
3 
YO 
F 
4 
ZO 
F 
5 
XL 
F 
6 
YL 
F 
7 
ZL 
F 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
8 
CIDL 
I 
0 
4 
5 
6 
7 
8 
Card 2 for <BLANK> Keyword Option. 
  Card 2 
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
3 
ZP 
F 
Default 
0.0 
0.0 
0.0
*DEFINE 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME 
C 
none 
  VARIABLE   
DESCRIPTION
CID 
Coordinate system ID.  A unique number has to be defined. 
XO 
YO 
ZO 
XL 
YL 
ZL 
CIDL 
XP 
YP 
ZP 
X-coordinate of origin. 
Y-coordinate of origin. 
Z-coordinate of origin. 
X-coordinate of point on local x-axis. 
Y-coordinate of point on local x-axis. 
Z-coordinate of point on local x-axis. 
Coordinate  system  ID  applied  to  the  coordinates  used  to  define
the current system.  The coordinates X0, Y0, Z0, XL, YL, ZL, XP,
YP,  and  ZP  are  defined  with  respect  to  the  coordinate  system
CIDL. 
X-coordinate of point in local x-y plane. 
Y-coordinate of point in local x-y plane. 
Z-coordinate of point in local x-y plane. 
FILENAME 
Name  of  the  IGES  file  containing  three  curves  . 
Remarks: 
1.  The  coordinates  of  the  points  must  be  separated  by  a  reasonable  distance  and 
not co-linear to avoid numerical inaccuracies.
Airbag
Application
Boundary
Constrained
Contact
Damping
Database
Define
Box
Coordinate
Vector
Elements
Initial
Load
Rigidwall
Set Data
Show
Cre
Mod
Del
Global
Local
Label: None
Coord
Type
*SYSTEM
Position
Node
New ID
C_Element
C_Edge
CID
Title
N+Xaxis
Nodes
TRAN
ROTA
Geopts
Refl
Origin
X-Axis
XYP
Avg_Cen
3PtCircle
C_Cur/Surf
Geometry
Compute
X:
Y:
Z:
Origin
XYPlane
Clear
AlongX
AlongY
AlongZ
Apply
Done
Cancel
NID
Create
Create Position
All
None
Rev
AList
Apply
Cancel
Write
Done
Create Entity
Figure 15-4.  LS-PrePost4.0 Dialog for defining a coordinate system. 
2.  Care must be taken to avoid chains of coordinate transformations because there 
is no guarantee that they will be executed in the correct order. 
3.  LS-PrePost.  A coordinate system can be created using the dialog box located 
at  Model (main  window) → CreEnt → Define   → Coordinate.  
This  will  activate  a  Define  Coordinate  dialog  in  the  right  pane.    Select  the  Cre 
radio  button  at  the  top  of  the  right  pane,  and  set  the  type  dropdown  to 
*SYSTEM.    The  next  set  of  radio  buttons  (below  the  title  input  box)  sets  the 
method used to define the coordinate system.  See Figure 15-4. 
a)  The N+Xaxis method generates a coordinate system from based on: 
i) 
ii) 
a user specified origin, 
one of the three global axes (this is a severe restriction), and 
iii)  a 3rd point.
N+Xaxis
Nodes
TRAN
ROTA
Geopts
Refl
Origin
X-Axis
XYP
Origin
X-Axis
XYPlane
Direction X
Clear
 Figure 15-5.  Subset of Create Entity dialog for both Nodes and Geopts methods.
The 3rd point, together with the specified global axis defines the new sys-
tem’s x-y plane.  The remaining axes are derived using orthogonality and 
right-handedness.    This  method  requires  the  user  to  pick  two  points 
which involves the Create Position dialog box, as shown in the left frame 
of Figure 15-4. 
NOTE:  After  defining  each  point  in  the  Create  Position  dialog,  it  is  very 
important  to  use  the  done  button.    The  Create  Entity  dialog  stays 
up and remains interactive while the Create Position dialog is also 
up and interactive.  This can be confusing.  Returning to the Cre-
ate Entity dialog without choosing done is a common mistake. 
b)  The node method generates a coordinate system from three points: 
i) 
The first point specifies the origin. 
ii)  The first and second points together specify the x-axis. 
iii)  The three points together specify the x-y plane of the new coordi-
nate system.  The y and z axis are derived from orthogonality and 
right-handedness. 
c)  The Geopts option generates the new coordinate system from a global axis 
and two points.  With this method the new system’s z-axis is set from the 
Direction drop-down.  This new system’s x-y plane is, then, orthogonal to 
the chosen direction.  The remaining two points serve to define the origin 
and  the  x-axis  (by  projecting  the  second  point).    This  option  is  useful  for 
metal forming application, since, often times, only the z-axis is important 
while the while the x and y axes are not.
Longest length curve
Local Z-axis
Mid-length curve
Local Y-axis
B3
B2
B1
Shortest length curve
Local X-axis
Figure  15-6.    Input  curves  (left).    The  generated  local  coordinate  system  is
written to the d3plot file as a part consisting of three beams (right). 
4. 
IGES.  When option, IGES, is used, three curves in the IGES format will be used 
to  define  a  local  coordinate  system.    IGES  curve  entity  types  126,  110  and  106 
are  currently  supported.    Among  the  three  curves,  the  longest  length  will  be 
made  as  local  Z-axis,  the  mid-length  will  be  Y-axis  and  the  shortest  length  X-
axis.  Suggested X, Y and Z-axis length is 100mm, 200mm and 300mm, respec-
tively. 
All  the  three  curves  must  have  one  identical  point,  and  will  be  used  for  the 
origin  of  the  new  local  coordinate  system.    The  coordinate  system  ID  for  the 
local system will be based on the IGES file name.  The IGES file name must start 
with a number, followed by an underscore “_”, or by a dot.  The number pre-
ceding the file name will be used as the new local coordinate system ID, which 
can then be referenced in *MAT_20 cards, for example.  
After  the  LS-DYNA  run,  three  beam  elements  of  a  new  PID  will  be  created  in 
place of the three curves representing the local X, Y, and Z-axis in the d3plot file 
for viewing in LS-PrePost.  See Figure 15-6. 
The following partial input contains an example in which the keyword is used 
to  create  a local coordinate system (CID = 25) from IGES input.   The IGES file 
named, 25_iges, contains three intersecting curves in one of the three supported 
IGES  entity  types.    The  example  demonstrates  using  the  IGES  coordinate  sys-
tem  (ID =  25)  to  specify  the  local  coordinate  system  for  a  rigid  body  (PID =  2, 
MID =  2).    The  keyword,  *BOUNDARY_PRESCRIBED_MOTION_RIGID_  LO-
CAL,  then  uses  this  local  coordinate  system  to  assign  velocities  from  load 
curves 3 and 5 for the rigid body motion in the local x-direction. 
*KEYWORD 
*DEFINE_COORDINATE_SYSTEM_IGES_TITLE 
Flanging OP25 
25_iges 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+---
-8 
*PART 
punch 
         2         2         2
*MAT_RIGID 
$      MID        RO         E        PR         N    COUPLE         M     
ALIAS 
         2 7.830E-09 2.070E+05      0.28 
$      CMO      CON1      CON2 
        -1        25    011111  
$LCO or A1        A2        A3        V1        V2        V3 
25 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+---
-8 
*BOUNDARY_PRESCRIBED_MOTION_RIGID_LOCAL 
$   typeID       DOF       VAD      LCID        SF       VID     DEATH     
BIRTH 
         2         1         0         3      -1.0         0   0.00241       
0.0 
         2         1         0         5      -1.0         0 0.0115243   
0.00241 
The keyword can be repeated for each new coordinate system if multiple coor-
dinate systems are needed. 
Revision information: 
This option is available starting in LS-DYNA Revision 62798.
*DEFINE_COORDINATE_VECTOR 
Purpose:  Define a local coordinate system with two vectors, see Figure 15-7.  The vector 
cross product, 𝑧 = 𝑥 × 𝑥𝑦, determines the z-axis.  The y-axis is then given by 𝑦 = 𝑧 × 𝑥.  If 
this  coordinate  system  is  assigned  to  a  nodal  point,  then  at  each  time  step  during  the 
calculation, the coordinate system is incrementally rotated using the angular velocity of 
the nodal point to which it is assigned. 
Card 
1 
Variable 
CID 
Type 
Default 
I 
0 
2 
XX 
F 
3 
YX 
F 
4 
ZX 
F 
5 
XV 
F 
6 
YV 
F 
7 
ZV 
F 
8 
NID 
I 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0. 
  VARIABLE   
DESCRIPTION
CID 
Coordinate system ID.  A unique number has to be defined. 
X-coordinate on local x-axis.  Origin lies at (0,0,0). 
Y-coordinate on local x-axis 
Z-coordinate on local x-axis 
X-coordinate of local x-y vector 
Y-coordinate of local x-y vector 
Z-coordinate of local x-y vector 
Optional nodal point ID.  The coordinate system rotates with the
rotation  of  this  node.    If  the  node  is  not  defined,  the  coordinate
system is stationary. 
XX 
YX 
ZX 
XV 
YV 
ZV 
NID 
Remarks: 
1.  These  vectors  should  be  separated  by  a  reasonable  included  angle  to  avoid 
numerical inaccuracies. 
2. 
Ideally, this nodal point should be attached to a rigid body or a structural part 
where  the  nodal  point  angular  velocities  are  meaningful.    It  should  be  noted 
that  angular  velocities  of  nodes  may  not  be  meaningful  if  the  nodal  point  is
attached  only  to  solid  elements  and  even  to  shell  elements  where  the  drilling 
degree of freedom may be singular, which is likely in flat geometries. 
xy
y 
x 
Figure 15-7.  Definition of the coordinate system with two vectors. 
Origin (0,0,0)
*DEFINE_CPM_BAG_INTERACTION 
Purpose:    To  model  energy  flow  from  a  master  airbag  to  a  slave  airbag.    The  master 
must be an active particle airbag and the slave a control volume (CV) airbag converted 
from a particle bag. 
To  track  the  flow  of  energy,  LS-DYNA  automatically  determines  which  vent  parts  are 
common  to  both  airbags.    At  each  time  step  the  energy  that  is  vented  through  the 
common vents is subtracted from the master and added to the slave.  In turn, the slave 
bag’s  pressure  provides  the  downstream  pressure  value  for  the  master  bag’s  venting 
equation.    While  this  model  accounts  for  energy  flow  from  master  to  slave  it  ignores 
flow from slave to master. 
If CHAMBER is used for slave CV bag, see remark 1. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Bag ID1 
Bag ID2 
Type 
I 
I 
Default 
none 
none 
  VARIABLE   
DESCRIPTION
Airbag ID of master CPM particle bag 
Airbag ID of slave CV bag switched from CPM bag 
Bag ID1 
Bag ID2 
Remarks: 
1.  Due  to  the  complexity  of  the  bookkeeping,  the  slave  may  have  several 
chambers  but  only  one  of  the  chambers  is  allowed  to  interact  with  the  master 
bag.    This  chamber  will  be  searched  automatically  through  the  commonly 
shared parts.
*DEFINE 
Purpose:    To  define  airbag  chambers  for  air  particle  initialization  or  chamber 
interaction. 
  Card 1 
Variable 
1 
ID 
Type 
I 
Default 
none 
2 
3 
4 
5 
6 
7 
8 
NCHM 
I 
0 
Chamber Definition Card Sets: 
Add NCHM chamber definition card sets.  Each chamber definition card set consists of 
a Chamber Definition Card followed by NINTER Interaction Cards. 
Chamber Definition Card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID1 
SID2 
NINTER 
CHM_ID 
Type 
I 
Default 
none 
I 
0 
I 
0 
I 
0 
Interaction Cards.  Add NINTER of these.  If NINTER = 0, skip this card.  
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID3 
ITYPE3 
TOCHM 
Type 
I 
I 
I 
Default 
none 
none 
none
P3 
P1 
Chamber 
997
Chamber 998
P2 
P4
Figure 15-8. 
  VARIABLE   
DESCRIPTION
ID 
Unique ID for this card 
NCHM 
Number of chambers defined in this card 
SID1 
SID2 
Part set defining all parts that constitute the chamber volume  
Part set defining the parts whose shell normals need to be flipped
(eg.  separation walls between chambers)  
NINTER 
Number of vent hole definition for chamber interaction. 
CHM_ID 
Chamber ID . 
SID3 
Set defining interaction between chambers 
ITYPE3 
Set type 
EQ.0: Part  
EQ.1: Part set 
TOCHM 
The chamber ID of the connected chamber.
*DEFINE 
1.  Each  chamber's  volume  is  calculated  based  on  the  part  normals  pointed 
inwards.  So SID1 would normally have parts with their shell normals pointing 
inwards.  But in some cases, parts may be shared by more than one chamber.  In 
this case, the shell orientation of certain part(s) may need to be flipped for the 
other  chambers  in  question.    In  such  cases,  SID2  can  be  used  to  flip  the  shell-
normals for specific parts. 
*SET_PART_LIST 
$#     sid 
         1 
$#    pid1      pid2      pid3      pid4 
         1         2         3         4 
*SET_PART_LIST 
$#     sid 
        20 
$#    pid1      pid2 
         1         2 
*DEFINE_CPM_CHAMBER 
$#      id      nchm 
      1234         2 
$#    sid1      sid2    ninter    chm_id 
        20         0         1       998 
$#    sid3    itype3     tochm 
         2         0       997 
$#    sid1      sid2    ninter    chm_id 
         1        20         1       997 
$#    sid3    itype3     tochm 
         2         0       998 
2.  Particles  with  different  chamber  ID  will  not  interact  in  particle  to  particle 
collision.  This feature will allow program to distinguish particles separated by 
a thin wall. 
3.  All  chambers  data  are  output  to  lsda  binout  database.    The  utility  “l2a”  can 
convert  it  into  abstat_chamber  ASCII  file  and  process  with  lsprepost  under 
abstat format
*DEFINE_CPM_GAS_PROPERTIES 
Purpose:  To define extended gas thermodynamic properties 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
Xmm 
Cp0 
Cp1 
Cp2 
Cp3 
Cp4 
Type 
I 
F 
F 
Default 
none 
none 
0. 
  Card 1 
1 
Variable 
μt0 
Type 
F 
Default 
0. 
2 
μt1 
F 
0. 
3 
μt2 
F 
0. 
F 
0. 
4 
μt3 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
5 
6 
7 
8 
μt4 
Chm_ID 
Vini 
F 
0. 
I 
0 
F 
0. 
  VARIABLE   
DESCRIPTION
ID 
Unique ID for this card 
Xmm 
Molar mass 
Cp0, …, Cp4 
Coefficients of temperature dependent specific heat with constant
pressure 
Cp(T) = Cp0 + Cp1 T + Cp2 T2 + Cp3 T3 + Cp4 T4 
μt0, …, μt4 
Coefficients of temperature dependent Joule-Thomson effect 
μt(T) = μt0 + μt1 T + μt2 T2  +  μt2 T3 + μt2 T4 
Chm_ID 
Chamber ID (remark 1) 
Vini 
Initial volume for user defined inflator (remark 1)
Example: 
*AIRBAG_PARTICLE 
$====1====$====2====$====3====$====4====$====5====$====6====$====7====$====8==== 
      1010         1      1011         1         0       0.0       0.0         1 
    100000         0         1     300.0   1.0e-04         1 
         1         1         1 
        61         0       1.0         0         0         1       0.0 
   1.0E-04     300.0     -9900 
       651       653     -9910 
   3000001       1.0 
$==================================================== 
*DEFINE_CPM_GAS_PROPERTIES 
$====1====$====2====$====3====$====4====$====5====$====6====$====7====$====8==== 
      9900 2.897E-02 2.671E+01 7.466E-03-1.323E-06 
      9910   4.0E-03     20.79 
   -610.63   -0.0926 
Remark: 
1.If  Chm_ID  and  Vini  are  defined.    This  gas  property  will  be  used  in  the  user_
inflator  routine  which  is  provided  in  the  dyn21b.f  of  general  usermat  package.  
The code will give current chamber volume, pressure, temperature and time step 
and  expect  returning  value  of  change  of  chamber,  burned  gas  temperature  and 
mass flow rate to feedback to the code for releasing particles.  All state data for 
this chamber will be output binout under abstat_chamber subdirectory.
Purpose:  To define extended vent hole options 
*DEFINE_CPM_VENT 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
C23 
LCTC23 
LCPC23 
ENH_V 
PPOP 
C23UP 
IOPT 
Type 
I 
F 
I 
I 
I 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
  Card 2 
Variable 
Type 
Default 
1 
JT 
I 
0 
2 
3 
4 
5 
6 
7 
8 
IDS1 
IDS2 
IOPT1 
PID1 
IPD2 
VANG 
I 
I 
I 
I 
I 
F 
none 
none 
none 
none 
none 
0. 
  VARIABLE   
DESCRIPTION
ID 
C23 
Unique ID for this card 
Vent  hole  coefficient. 
parameter.  (Default 1.0) 
  This 
is  the  Wang-Nefske 
leakage 
LCTC23 
Load curve defining vent hole coefficient as a function of time. 
LCPC23 
ENH_V 
Load  curve  defining  vent  hole  coefficient  as  a  function  of
pressure. 
Enhance venting option.  (Default 0).  However if Joule-Thomson 
effect is considered, the option will set to 1 automatically. 
EQ.0: disable 
EQ.1: enable 
PPOP 
Pressure  difference  between  interior  and  ambient  pressure  to
open the vent hole.  Once the vent is open then it will stay open.
VARIABLE   
C23UP 
DESCRIPTION
Scale  factor  of  C23  while  switching  from  CPM  to  uniform
pressure calculation. 
IOPT 
Directional venting: 
EQ.1: 
In shell normal 
EQ.2:  Against shell normal 
One-way venting: 
EQ.10:  In shell normal 
EQ.20:  Against shell normal 
Special vent option:: 
EQ.100:  Enable  compression  seal  vent.    Vent  area  is  adjusted
according to the formula below.  See Remark 1. 
𝐴vent = max(𝐴current − 𝐴0, 0) 
EQ.200:  Enable  push-out  vent.    Particle  remains  active  while 
going through this external vent within the range of 2
times of its characteristic length, 𝑙vent. 
𝑙vent = √𝐴vent 
JT 
Include  the  Joule-Thomson  effect.    When  the  Joule-Thomson 
effect is enabled ENH_V is automatically set to 1 (enable). 
EQ.0:  disable 
EQ.1: use part pressure 
EQ.2: use chamber pressure 
IDS1 
IDS2 
IOPT1 
PID1, PID2 
JT's up stream condition part ID/chamber ID 
JT's downstream condition part ID/chamber ID 
Upstream chamber ID for one-way vent hole.  This  will help the 
code to determine the probability function. 
When  specified  the  vent  probability  function  is  evaluated  from
the  difference  of  local  part  pressures  (between  PID1  and  PID2)
instead  of  the  usual  calculation  involving  the  chamber  pressure.
This  option  is  usually  used  for  vents  near  a  long  sleeve  which
causing unrealistic venting using chamber pressure alone.
VANG 
*DEFINE_CPM_VENT 
DESCRIPTION
Cone  angle  in  degrees.    Particle  goes  through  this  vent  will  be
redirection  based  on  this  angle.    This  option  is  only  valid  with 
internal vent. 
GT.0:  cone angle (maximum 270) 
EQ.0: disabled (Default) 
LT.0:  direction follows the vent normal  
Remarks: 
1.  Compression  Seal  Vent  Model.    In  order  to  evaluate  bag  state  variables 
correctly,  the  CPM  domain  needs  to  be  a  closed  surface  for  the  volume  to  be 
well-defined.  If the model contains a flap vent which is free to open and close, 
this option will correctly maintain the bag’s integrity. 
Example: 
*AIRBAG_PARTICLE 
$====1====$====2====$====3====$====4====$====5====$====6====$====7====$====8==== 
      1010         1      1011         1         0       0.0       0.0         1 
    100000         0         1     300.0   1.0e-04         1 
         1         1         1 
        61         0     -9910 
   1.0E-04     300.0  2.897E-2  2.671E+1  7.466E-3 -1.323E-6 
      1000      1001    4.0E-3     20.79 
   3000001       1.0 
$==================================================== 
*DEFINE_CPM_VENT 
$====1====$====2====$====3====$====4====$====5====$====6====$====7====$====8==== 
      9910       1.0         0         0         1       0.0 
         1        51         2
*DEFINE 
Purpose:    Define  a  curve  [for  example,  load  (ordinate  value)  versus  time  (abscissa 
value)], often loosely referred to as a load curve.  The ordinate may represent something 
other than a load however, as in the case of curves for constitutive models. 
In the case of constitutive models, *DEFINE_CURVE curves are rediscretized internally 
with equal intervals along the abscissa for fast evaluation.  Rediscretization is not used 
when  evaluating  loading  conditions  such  as  pressures,  concentrated  forces,  or 
displacement boundary conditions . 
The curve rediscretization algorithm was enhanced for the 2005 release of version 970.  
In certain cases the new load-curve routines changed the final results enough to disrupt 
benchmarks.  For validated models, such as barriers and occupants, requiring numerical 
consistency, there are keyword options for reverting to the older algorithms. 
Available options include: 
<OPTION> 
3858 
5434a 
which correspond to the first releases of version 970 and the 2005 release, respectively.   
Since input errors and wrong results are sometimes related to load curve usage, a “Load 
curve  usage”  table  is  printed  in  the  d3hsp  file  after  all  the  input  is  read.    This  table 
should  be  checked  to  ensure  that  each  curve  ID  is  referenced  by  the  option  for  which 
the curve is intended. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
SIDR 
SFA 
SFO 
OFFA 
OFFO 
DATTYP 
LCINT 
Type 
I 
Default 
none 
I 
0 
F 
1. 
F 
1. 
F 
0. 
F 
0. 
I 
0 
I
Point Cards.  Put one pair of points per card (2E20.0).  Input is terminated at the next 
keyword (“*”) card. 
Card 2… 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
A1 
O1 
Type 
E20.0 
E20.0 
Default 
0.0 
0.0 
  VARIABLE   
LCID 
SIDR 
SFA 
SFO 
OFFA 
OFFO 
DESCRIPTION
Load  curve  ID.    Tables    and  load  curves 
may  not  share  common  ID's.    LS-DYNA  allows  load  curve  ID's 
and table ID's to be used interchangeably.  A unique number has
to be defined. 
Flag controlling use of curve during dynamic relaxation.  SIDR set
to  1  or  2  will  activate  a  dynamic  relaxation  phase  unless  IDR-
FLG = -999 in *CONTROL_DYNAMIC_RELAXATION. 
EQ.0: load  curve  used  in  normal  analysis  phase  only  or  for
other applications, 
EQ.1: load curve used in dynamic relaxation phase but not the
normal  analysis phase, 
EQ.2: load curve applies to both dynamic relaxation phase and
normal analysis phase. 
Scale  factor  for  abscissa  value.    This  is  useful  for  simple
modifications. 
EQ.0.0: default set to 1.0. 
Scale factor for ordinate value (function).  This is useful for simple
modifications. 
EQ.0.0: default set to 1.0. 
Offset for abscissa values, see explanation below. 
Offset for ordinate values (function), see explanation below.
DATTYP 
*DEFINE 
DESCRIPTION
Data  type.    This  affects  how  offsets  are  applied  .  
EQ.-2:  for  fabric  stress  vs.    strain  curves  (*MAT_FABRIC)  as 
described   
 below. 
EQ.0:  general  case  for  time  dependent  curves,  force  versus
displacement curves and stress strain curves 
EQ.1:  for general (𝑥, 𝑦) data curves whose abscissa values do 
not increase monotonically 
EQ.6:  for  general  (𝑟, 𝑠)  data  (coordinates  in  a  2D  parametric 
space)  whose  values  do  not  increase  monotonically.
Use  for  definition  of  trimming  polygons  for  trimmed
NURBS 
(*ELEMENT_SHELL_NURBS_PATCH, 
NL.GT.0) 
LCINT 
The  number  of  discretization  points  to  use  for  this  curve.   If  0  is
input, the value of LCINT from *CONTROL_SOLUTION will be 
used. 
A1, A2, … 
Abscissa values.  See remarks below. 
O1, O2, … 
Ordinate (function) values.  See remarks below. 
Remarks: 
1.  Warning  Concerning  Rediscretization.    For  constitutive  models,  LS-DYNA 
internally  rediscretizes  the  curve  with  uniform  spacing  to  bypass  searching 
during evaluations.  The major drawback of this algorithm is that any detail in 
the  curve  on  a  scale  finer  than  the  uniform  rediscretization  grid  will  be 
smoothed-out and lost.  It is, therefore, important to avoid placing a single point off 
at some value approaching infinity.  The lone point at infinity will cause the resolu-
tion  of  the  uniform  grid  to  be  coarse  relative  to  the  other  points,  causing  the 
rediscretized curve to be, possibly, featureless. 
Therefore,  when  defining  curves  for  constitutive  models,  points  should  be 
spaced as uniformly as possible.  Also, since the constitutive model curves are 
extrapolated, it is important to ensure that extrapolation does not lead to physi-
cally meaningless values, such as a negative flow stress.  Conversely, extrapola-
tion can be exploited to control the results of evaluations at points far from the 
input data.
The number of points in each rediscretized curve is controlled by the parameter 
LCINT  in  *CONTROL_SOLUTION.    By  changing  LCINT  to  a  value  greater 
than the default of 100, the rediscretized curves may better resemble the input 
curves.  The data points of the rediscretized curves are written to messag and 
d3hsp if the parameter IPCURV is set to 1 in *CONTROL_OUTPUT. 
2.  Scaling.  The load curve values are scaled after the offsets are applied, i.e.: 
Abscissa  value = SFA × (Defined  value + OFFA) 
Ordinate  value = SFO × (Defined  value + OFFO) 
3.  DATTYP.    The  DATTYP  field  controls  how  the  curve  is  processed  during  the 
calculation. 
a)  For  DATTYP =  0  positive  offsets  may  be  used  when  the  abscissa  repre-
sents time, since two additional points are generated automatically at time 
zero and at time 0.999 × OFFA  with the function values set to zero. 
b)  If  DATTYP =  1,  then  the  offsets  do  not  create  these  additional  points.  
Negative offsets for the abscissa simply shifts the abscissa values without 
creating additional points. 
c)  For *MAT_FABRIC material with FORM = 4, 14, -14, or 24, set DATYP = -
2 to define stress vs.  strain curves using engineering stress and strain ra-
ther the 2nd Piola-Kirchhoff stress and Green strain. 
4.  Context  Dependent  Extrapolation.    Load  curves  are  not  extrapolated  by  LS-
DYNA  for  applied  loads  such  as  pressures,  concentrated  forces,  displacement 
boundary conditions, etc.  Function values are set to zero if the time, etc., goes 
off scale.  Therefore, extreme care must be observed when defining load curves.  
In  the  constitutive  models,  extrapolation  is  employed  if  the  values  on  the  ab-
scissa go off scale. 
5.  Restart.    The  curve  offsets  and  scale  factors  are  ignored  during  restarts  if  the 
curve is redefined.  See *CHANGE_CURVE_DEFINITION in the restart section.
*DEFINE_CURVE_BOX_ADAPTIVITY 
Purpose:  To define a polygon adaptive box in sheet metal forming, applicable to shell 
elements.  This keyword is used together with *CONTROL_ADAPTIVE.  Other related 
keyword is *DEFINE_BOX_ADAPTIVE. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
PID 
LEVEL 
DIST1 
Type 
I 
I 
I 
F 
Default 
none 
none 
none 
none 
Point Cards.  Include as many as necessary.  This input ends at the next keyword (“*”) 
card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
X 
F 
Y 
F 
Z 
F 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION
ID 
Curve ID; must be unique.  The curve must be closed: its first and
last point must coincide. 
PID 
Sheet blank Part ID, as in *PART. 
LEVEL 
Adaptive  refinement  levels,  similar  to  ‘MAXLVL’  in  *CON-
TROL_ADAPTIVE.
DIST1 
*DEFINE_CURVE_BOX_ADAPTIVITY 
DESCRIPTION
Extended depths in Z  for a polygon box defined by Card 2, 3, 4, 
etc.      Currently  this  variable  must  be  input  as  a  negative  value.
The  box  depth  in  Z  will  be  extended  in  –Z  direction  by  Zmin-
abs(DIST1)  and  in  +Z  direction  by  Zmax+abs(DIST1).    The  XYZ 
data  pairs  formed  with  Card  2,  3,  4,  etc.    will  be  automatically 
closed  to  create  the  polygon  box.    Zmin  and  Zmax  are  the
minimum and maximum Z-coordinates in all the data pairs.  
X 
Y 
Z 
X-coordinate of a point on the curve. 
Y-coordinate of a point on the curve. 
Z-coordinate of a point on the curve. 
Remarks: 
Within  the  polygon,  the  variable  LEVEL  has  priority  over  MAXLVL  in  *CONTROL_-
ADAPTIVE  but  limited  to  minimum  element  size  controlled  by  ADPSIZE.    A  larger 
LEVEL  (than  MAXLVL)  value  will  enable  more  mesh  refinement  within  the  polygon, 
up to the size defined by ADPSIZE, while  meshes outside of the  box refined less  by a 
smaller  MAXLVL  value.    However,  mesh  refinement  when  LEVEL > MAXLVL  is  not 
recommended.    The  appropriate  way  of  using  this  keyword  (and  *DEFINE_BOX_-
ADAPTIVE)  is  to  define  the  polygon  box  excluding  the  local  areas  of  interest  so 
refinement  inside  the  local  areas  will  be  controlled  by  MAXLVL  while  outside  of  the 
area to be controlled by LEVEL, and in this case MAXLVL > LEVEL, as shown in Figure 
15-9.    The  advantage  of  using  this  keyword  is  obvious  when  compared  with  multiple 
boxes needed when defining local adaptive refinement with keyword *DEFINE_BOX_-
ADPATIVE  (Figure  15-10).    It  is  noted  that  ADPSIZE  is  a  “global”  variable,  meaning 
final refined element sized, regardless of the values set for MAXLVL or LEVEL, cannot 
be smaller than what is defined by ADPSIZE. 
The  3-D  curve  (closed  polygon)  defined  by  XYZ  data  pairs  should  be  near  the  sheet 
blank in Z after the blank is auto-positioned in the beginning of a simulation.  Similar to 
*DEFINE_BOX_ADAPTIVE,  only  the  elements  on  the  sheet  blank  initially  within  the 
polygon will be considered for use with this keyword.  Local coordinate system is not 
supported at the moment. 
The 3-D curve can be converted from IGES format to format required here following the 
procedure outlined in keyword *INTERFACE_BLANKSIZE_{OPTION}. 
A partial keyword example is provided below, where inside the polygon mesh has no 
refinement  (LEVEL = 1),  while  outside  of  the  box  the  mesh  is  refined  5  levels
(MAXLVL = 5).  The final minimum element size is defined as 0.4.  It is noted that the 
first point and last point of the polygon are the same, closing the polygon box. 
*CONTROL_ADAPTIVE 
$  ADPFREQ    ADPTOL    ADPOPT    MAXLVL    TBIRTH    TDEATH     LCADP    IOFLAG 
   &adpfq1       5.0         2         5       0.0 1.000E+20                   1 
$  ADPSIZE    ADPASS    IREFLG    ADPENE     ADPTH    MEMORY    ORIENT     MAXEL 
       0.4         1         0   &lookfd       0.0                   0         0 
$  IADPE90              NCFREQ    IADPCL    ADPCTL    CBIRTH    CDEATH     LCLVL 
        -1 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*DEFINE_CURVE_BOX_ADAPTIVITY 
$       ID       PID     LEVEL     DIST1 
        99         1         1     -25.0 
$(3E20.0): 
          -59.573399           -6.698870          -40.224651 
          -90.728516           24.456253          -40.224651 
... 
          -23.213169           18.088070          -10.954337 
           14.353654           16.130911          -10.954337 
          -31.070744           -5.785467          -40.487387 
          -59.573399           -6.698870          -40.224651 
Revision information: 
This  feature  is  available  in  SMP  only,  and  in  LS-DYNA  Revision  81918  and  later 
releases.
Zmax+abs(DIST1)
Adaptivity within the polygon is  controlled 
by LEVEL in 
*DEFINE_CURVE_BOX_ADAPTIVITY
Zmin - abs(DIST1)
Adaptivity in flanging area outside of 
the polygon is controlled by MAXLVL 
in *CONTROL_ADAPTIVE, and 
MAXLVL > LEVEL.
Figure 15-9.  Defining an adaptive polygon box
Adaptivity within these boxes is  
controlled by LEVEL in 
*DEFIN_BOX_ADAPTIVE
Adaptivity in flanging area along the 
hood line is controlled by MAXLVL 
in *CONTROL_ADAPTIVE, and 
MAXLVL > LEVEL.
Figure 15-10.  Defining adaptive boxes
*DEFINE_CURVE_COMPENSATION_CONSTRAINT_OPTION 
Purpose:  This keyword with the two options allows for the definition of a localized die 
face region for springback compensation of stamping tools. 
Options available include: 
BEGIN 
END 
NOTE:  *DEFINE_CURVE_COMPENSATION_CONSTRAINT_BEGIN 
and  *DEFINE_CURVE_COMPENSATION_CONSTRAINT_END 
are not valid in the context of a general keyword input deck.  In-
stead, they may only be used inside of an *INCLUDE_COMPEN-
SATION_CURVE include file. 
The required option, which must be either BEGIN or END, distinguishes between two 
different  closed  curves,  which,  when  taken  together  identify  a  portion  of  the  die 
wherein  springback  compensation  is  applied,  and  a  transition  region  for  which 
compensation smoothly tapers off. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CRVID 
INOUT 
TYPE 
Type 
Default 
I 
0 
I 
0 
I 
none 
Point  Cards.    Include  as  many  as  necessary  (3E16.0).    This  input  ends  at  the  next 
keyword (“*”) card.  Only the projection of this curve onto the 𝑥-𝑦 plane is used. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
X 
F 
Y 
F 
Z 
F 
Default 
0.0 
0.0 
0.0
A perfect sphere surface
An area of impection
(to be compensated)
Section A-A
Begin curve
Transition area
End curve
  VARIABLE   
CRVID 
Figure 15-11.  Local area compensation. 
DESCRIPTION
Curve ID; must be unique.  The curve must be closed: its first and
last point must coincide. 
INOUT 
Flag to indicate local area to be compensated: 
EQ.0:  For  this  option,  the  compensated  region  of  the  die
consists of all points for which the projection onto the 𝑥-𝑦
plane  is  exterior  to  the  projection  of  the  BEGIN  curve.
The  projection  of  the  END  curve  is  assumed  exterior  to
the BEGIN curve.  The transition region, then, consists of 
all  die  points  for  which  the  projection  is  between  the
BEGIN and END curves.  All other points on the die are
uncompensated. 
EQ.1:  For  this  option,  the  compensated  region  of  the  die
consists of all points for which the projection onto the 𝑥-𝑦
plane  is  interior  to  the  projection  of  the  BEGIN  curve.
The  projection  of  the  END  curve  is  assumed  exterior  to
the BEGIN curve.  The transition region, then, consists of
all  die  points  for  which  the  projection  is  between  the
BEGIN and END curves.  All other points on the die are 
uncompensated.  See Figure 15-11. 
TYPE 
Type code - must be “0”. 
X 
Y 
𝑥-coordinate of a point on the curve. 
𝑦-coordinate of a point on the curve.
*DEFINE_CURVE_COMPENSATION_CONSTRAINT 
DESCRIPTION
Z 
𝑧-coordinate of a point on the curve. 
Motivation: 
Sometimes springback occurs in a localized region of the die face.  Since other parts of 
the die face are better left undisturbed, a localized compensation makes the most sense 
to  bring  the  part  shape  back  to  the  design  intent.    A  typical  such  example  will  be  the 
front portion along the grill and headlamp, or the rear portion along the windshield of a 
trimmed  hood  inner  panel.    A  decklid  (or  trunk  lid)  inner  also  exhibits  the  similar 
needs.    Once  the  localized  areas  are  identified,  iterative  compensation  scheme  may  be 
employed  within  this  localized  region  to  bring  the  springback  panel  back  to  design 
shape. 
Modeling details: 
Referring  to  Figure  15-11,  the  keywords  *COMPENSATION_CONSTRAINT_BEGIN 
and *COMPENSATION_CONSTRAINT_END must be used together in a file, which in 
turn  will  be  included  in  keyword  *INCLUDE_COMPENSATION_CURVE.    The 
keyword “BEGIN” precedes the keyword “END”, each is defined by discrete points.  In 
addition, each curve must form a closed loop.  The area formed between the two curves 
is  a  transition  area,  and  will  be  affected  in  the  compensated  tooling.    LS-PrePost4.0 
under Curve → Merge → Multiple Method, multiple disconnected curves can be joined 
together, and output in “.xyz” format required here. 
The curve can be a 3-D piecewise linear curve with coordinates in 𝑥, 𝑦 and 𝑧.  However, 
𝑧-coordinates  are  ignored;  meaning  the  tooling  to  be  compensated  must  be  positioned 
so  draw  direction  is  in  global  𝑧;  otherwise  error  will  occur.    In  addition,  it  is  assumed 
that both “blank before springback” and “blank after springback” will be smaller than 
rigid tools in dimension.  It is further noted the rigid tool meshes should be discretized 
fine enough to provide enough degrees of freedom for the compensation. 
Application example – single region: 
A  complete  input  deck  is  provided  below  for  a  local  compensation  simulation.    The 
keyword files state1.k and state2.k consist model (nodes and elements) information of 
the blank before and after springback, respectively.  It is noted here that if the blank is 
adaptively refined, the adaptive constraints must be included in the keyword files.  The 
keyword file tools.k consists the stamping tools (with PID 1, 2, 3 and 4) all positioned in 
home position.  The keyword file curvesxy.xyz consists keywords “BEGIN” and “END” 
defining the two closed-loop curves used to define a localized area.  
*KEYWORD
*TITLE 
LS-Dyna971 Compensation Job 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*INTERFACE_COMPENSATION_NEW 
$   METHOD        SL        SF     ELREF     PSIDm     UNDCT    ANGLE   NOLINEAR 
         6    10.000     0.700         0         1         0        0          1 
*INCLUDE_COMPENSATION_BLANK_BEFORE_SPRINGBACK 
state1.k 
*INCLUDE_COMPENSATION_BLANK_AFTER_SPRINGBACK 
state2.k 
*INCLUDE_COMPENSATION_DESIRED_BLANK_SHAPE 
state1.k 
*INCLUDE_COMPENSATION_COMPENSATED_SHAPE 
state1.k 
*INCLUDE_COMPENSATION_CURRENT_TOOLS 
tools.k 
*INCLUDE_COMPENSATION_CURVE 
curvesxy.xyz 
*SET_PART_LIST 
         1 
1,2,3,4 
*END 
A portion of the file curvesxy.xyz is shown below,  
*KEYWORD 
*DEFINE_CURVE_COMPENSATION_CONSTRAINT_BEGIN 
$      CID    IN/OUT      TYPE 
         1         1         0 
    -1.86925e+02     1.83338e+03    -1.55520e+01 
    -1.83545e+02     1.83003e+03    -1.55469e+01 
    -1.80162e+02     1.82668e+03    -1.55428e+01 
    -1.91811e+02     1.83884e+03    -1.56014e+01 
    -1.90187e+02     1.83701e+03    -1.55852e+01 
    -1.88560e+02     1.83519e+03    -1.55688e+01 
    -1.86925e+02     1.83338e+03    -1.55520e+01 
*DEFINE_CURVE_COMPENSATION_CONSTRAINT_END 
$      CID    IN/OUT      TYPE 
         2         1         0 
    -4.07730e+02     1.61371e+03    -8.04858e+01 
    -3.84480e+02     1.59890e+03    -7.99169e+01 
    -3.61193e+02     1.58423e+03    -7.93471e+01 
    -3.37832e+02     1.56984e+03    -7.87756e+01 
    -4.49289e+02     1.67556e+03    -8.04582e+01 
    -4.35672e+02     1.65473e+03    -8.05162e+01 
    -4.21764e+02     1.63396e+03    -8.05530e+01 
    -4.07730e+02     1.61371e+03    -8.04858e+01 
*END
Compensated tool
Target mesh
Springback mesh
Section A-A
Figure 15-12.  Local compensation details. 
It is noted the first point and last point are exactly the same, forming a closed loop.  In 
Figure 15-11, local area compensation is to be performed in the center portion of a rigid 
sphere.  Based on springback and target meshes, the compensated tool mesh is obtained 
and  smooth  transition  areas  are  achieved,  Figure  15-12.    Here  the  compensation  scale 
factor of 0.7 is used. 
Application example – multiple regions: 
Multi-region localized compensation is also possible by defining multiple pairs of  the 
BEGIN  and  END  versions  of  this  keyword,  each  forming  a  localized  region.    For 
example,  for  localized  compensation  of  two  regions,  the  file  curvesxy.xyz  will  read  as 
follows, 
*KEYWORD 
*DEFINE_CURVE_COMPENSATION_CONSTRAINT_BEGIN 
$      CID    IN/OUT      TYPE 
         1         1         0 
     3.67967e+02     1.63423e+03    -6.98532e+01 
     3.60669e+02     1.62992e+03    -6.92921e+01 
     3.53586e+02     1.62525e+03    -6.88777e+01 
⋮ 
⋮ 
⋮ 
*DEFINE_CURVE_COMPENSATION_CONSTRAINT_END 
$      CID    IN/OUT      TYPE 
         2         1         0 
     4.12534e+02     1.75537e+03    -5.83975e+01 
     3.98853e+02     1.75264e+03    -5.58860e+01 
     3.85292e+02     1.74921e+03    -5.35915e+01 
⋮ 
⋮ 
⋮ 
*DEFINE_CURVE_COMPENSATION_CONSTRAINT_BEGIN 
$      CID    IN/OUT      TYPE 
         3         1         0 
    -4.37478e+02     2.67393e+03    -1.70421e+02 
    -4.45605e+02     2.67209e+03    -1.71724e+02 
    -4.53649e+02     2.66985e+03    -1.72894e+02 
⋮ 
⋮ 
⋮ 
*DEFINE_CURVE_COMPENSATION_CONSTRAINT_END 
$      CID    IN/OUT      TYPE 
         4         1         0 
    -4.49426e+02     2.79057e+03    -2.18740e+02 
    -4.63394e+02     2.78749e+03    -2.20955e+02
Section B-B
Compensated tool
Target mesh
Section B-B
Springback mesh
Figure 15-13.  Multi-region local compensation. 
    -4.77223e+02     2.78370e+03    -2.22938e+02 
⋮ 
*END 
⋮ 
⋮ 
Figure  15-13  (top)  shows  an  example  of  two  localized  areas  of  the  sphere  to  be 
compensated.  The compensation results are shown in Figure 15-13 (bottom).  Again, a 
compensation scale factor of 0.7 was used and smooth transition areas are achieved. 
Revision information: 
This feature is available in double precision version of LS-DYNA starting in Revision 62038.  
Multi-region  localized  compensation  is  available  starting  in  Revision  66129  and  later 
releases.    In  addition,  prior  to  Revision  66129,  all  keywords  must  be  capitalized.    Also, 
official release version starting in R7.1.1 (double precision) can be used.
*DEFINE_CURVE_DRAWBEAD 
Purpose:    This  keyword  simplifies  the  definition  of  a  draw  bead,  which  previously 
required the use of many keywords. 
NOTE:  This  option  has  been  deprecated  in  favor  of  *DE-
FINE_MULTI_DRAWBEADS_IGES. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CID 
TCTYPE 
VID 
PID 
BLKID 
PERCT 
LCID 
Type 
I 
I 
I 
I 
I 
F 
I 
Default 
none 
none 
none 
none 
none 
0.0 
none 
Point  Cards.    For  TCTYPE = 1  define  points  on  the  curve.    Input  is  terminated  at  the 
next keyword (“*”) card. 
4 
5 
6 
7 
8 
  Card 2 
Variable 
1 
CX 
Type 
F 
2 
CY 
F 
3 
CZ 
Default 
0.0 
0.0 
IGES Card.  For TCTYPE = 2 set an IGES file. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME 
C 
none
VARIABLE   
DESCRIPTION
CID 
Draw bead curve ID; must be unique. 
TCTYPE 
Flag to indicate input curve data format: 
EQ.1: XYZ data, 
EQ.2: IGES format data. 
VID 
PID 
Vector ID, as defined by *DEFINE_VECTOR.  This vector is used 
to project the supplied curves to the rigid tool, defined by the PID
below. 
Part  ID  of  a  rigid  tool  to  which  the  curves  are  projected  and 
attached. 
BLKID 
Part ID of the blank. 
PERCT 
Draw bead lock percentage or draw bead force. 
GT.0: Percentage  of  the  full  lock  force  for  the  bead  defined.
This is the ratio of desired restraining force over the full
lock force.  The value should be between 0.0 and 100.0. 
LT.0:  Absolute value is the draw bead force. 
LCID 
Load  curve  ID  defining  material  hardening  curve  of  the  sheet 
blank, BLKID. 
CX, CY, CZ 
Points on the curve. 
FILENAME 
IGES file name. 
Remarks: 
1.  This feature implements the following input algorithm for drawbeads: 
a)  It reads a draw bead curve in either XYZ or IGES format 
b)  projects the curve to the rigid tool specified 
c)  creates extra node set and attaches it to the rigid tool. 
d)  With supplied material hardening curve (LCID), full lock force is calculat-
ed. 
There  is  no  need  to  define  *CONTACT_DRAWBEAD  and  *CONSTRAINED_-
RIGID_BODIES since they are treated internally within the code.
2.  The  “curve”  menu  in  LS-PrePost  can  be  used  to  break  or  join  multiple 
disconnected curves, and output in either ‘XYZ’ or IGES format. 
3.  The following partial keyword example defines a draw bead curve ID 98 (IGES 
file “bead1.iges”) to restrain blank part ID 63.  Full lock force is calculated from 
the strain hardening curve ID 400.  The draw bead is projected along vector ID 
991, and is attached to a rigid tool of part ID 3. 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+---
-8 
*KEYWORD 
*DEFINE_VECTOR 
991,0.0,0.0,0.0,0.0,0.0,10.0 
*DEFINE_CURVE_DRAWBEAD 
$      CID    TCTYPE       VID       PID     BLKID     PERCT      LCID 
        98         2       991         3        63    52.442       400 
bead1.iges 
*MAT_037 
$      MID        R0         E        PR      SIGY      ETAN         R     
HCLID 
         1  7.89E-09  2.00E+05       0.3     240.0                 1.6      
400 
*DEFINE_CURVE 
400 
0.0,240.0 
0.02,250.0 
... 
1.0, 350.0 
*END 
Revision information: 
This feature is available starting in LS-DYNA R5 Revision 62464.
*DEFINE 
Purpose:  Define a curve by optionally scaling and offsetting the abscissa and ordinates 
of another curve defined by the *DEFINE_CURVE keyword. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
RLCID 
SFA 
SFO 
OFFA 
OFFO 
Type 
I 
I 
F 
Default 
none 
none 
1. 
F 
1. 
F 
0. 
F 
0. 
  VARIABLE   
LCID 
DESCRIPTION
Load  curve  ID.    Tables    and  load  curve 
ID’s must be unique. 
RLCID 
Reference load curve ID. 
SFA 
SFO 
OFFA 
OFFO 
Scale  factor  for  abscissa  value  of  curve  ID,  RLCID.    This  value
scales the SFA value defined for RLCID. 
EQ.0.0: default set to 1.0. 
Scale  factor  for  ordinate  value  (function)  of  curve  ID,  RLCID.
This value scales the SFO value defined for RLCID. 
EQ.0.0: default set to 1.0. 
Offset for abscissa values.  This value is added to the OFFA value
defined for RLCID. 
Offset  for  ordinate  values  (function).    This  value  is  added  to  the
OFFO value defined for RLCID.
*DEFINE_CURVE_ENTITY 
Purpose:    Define  a  curve  of  straight  line  segments  and  circular  arcs  that  defines  an 
axisymmetric surface.  This curve can only be used with the keyword, *CONTACT_EN-
TITY for the load curve entity, GEOTYP = 11. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
SFA 
SFO 
SFR 
OFFA 
OFFO 
OFFR 
Type 
I 
F 
Default 
none 
1. 
F 
1. 
F 
1. 
F 
0. 
F 
0. 
F 
0. 
Point  Cards.    Put  one  point  per  card  (3E20.0,I20).    Include  as  many  cards  as  needed 
Input is terminated when a “*” card is found.  
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Ai 
F 
Oi 
F 
Ri 
F 
Default 
0.0 
0.0 
optional 
IFLAG 
I 
Required if 
|R1| > 0 
  VARIABLE   
LCID 
DESCRIPTION
Load  curve  ID.    Tables    and  load  curves 
may  not  share  common  ID's.    LS-DYNA  allows  load  curve  ID's 
and table ID's to be used interchangeably.  A unique number has
to be defined. 
SFA 
Scale factor for axis value.  This is useful for simple modifications.
EQ.0.0: default set to 1.0. 
SFO 
Scale  factor  for  radius  values. 
modifications. 
  This  is  useful  for  simple
EQ.0.0: default set to 1.0.
VARIABLE   
SFR 
DESCRIPTION
Scale  factor  for  circular  radius.    This  is  useful  for  simple
modifications. 
EQ.0.0: default set to 1.0. 
Offset for axis values, see explanation below. 
Offset for radius values, see explanation below. 
Offset for circular radius, see explanation below. 
Z-axis coordinates along the axis of rotation. 
Radial coordinates from the axis of rotation 
Radius  of  arc  between  points  (Ai,Oi)  and  (Ai+1,Oi+1).   If  zero,  a
straight line segment is assumed. 
Defined if |Ri| > 0.  Set to 1 if center of arc is inside axisymmetric
surface and to -1 if the center is outside the axisymmetric surface.
OFFA 
OFFO 
OFFR 
Ai 
Oi 
Ri 
IFLAG 
Remarks: 
1. 
The load curve values are scaled after the offsets are applied, i.e.: 
Axis value = SFA × (Defined value + OFFA) 
Radius value = SFO × (Defined value + OFFO) 
Circular value = SFR × (Defined value + OFFR)
*DEFINE_CURVE_FEEDBACK 
Purpose:    Define  information  that  is  used  as  the  solution  evolves  to  scale  the  ordinate 
values of the specified load curve ID.  This keyword is usually used in connection with 
sheet metal forming calculations. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
PID 
BOXID 
FLDID 
Type 
I 
I 
Default 
none 
none 
  Card 2 
1 
2 
I 
0 
3 
I 
none 
4 
5 
6 
7 
8 
Variable 
FSL 
TSL 
SFF 
SFT 
BIAS 
Type 
F 
F 
F 
F 
F 
Default 
none 
none 
1.0 
1.0 
0.0 
  VARIABLE   
DESCRIPTION
LCID 
PID 
BOXID 
FLDID 
FSL 
TSL 
ID number for load curve to be scaled. 
Active part ID for load curve control 
Box  ID.    Elements  of  specified  part  ID  contained  in  box  are
checked.  If the box ID is set to zero the all elements of the active
part are checked. 
Load curve ID which defines the flow limit diagram as shown in 
Figure 15-14. 
If  the    ratio,  𝑟 = εmajorworkpiece
factor for flow, SFF, is active. 
⁄
𝜀majorfld
exceeds  FSL,  then  scale 
Thickness  strain  limit.    If  the  thickness  strain  limit  is  exceeded,
then the  scale factor for thickening, SFT, is active.
εmnr = 0 
PLANE STRAIN εmjr
80
70
60
50
40
30
20
10
%
εmnr
εmjr
εmnr
εmjr
DRAW
STRETCH
-50
-40
-30
-20
-10
+10
+20
+30
+40
+50
% MINOR STRAIN
Figure 15-14.  Flow limit diagram. 
  VARIABLE   
DESCRIPTION
Scale factor for the flow limit diagram. 
Scale factor for thickening. 
Bias for combined flow and thickening.  Bias must be between -1 
and 1. 
SFF 
SFT 
BIAS 
Remarks: 
This  feature  scales  the  ordinate  values  of  a  load  curve  according  to  a  computed  scale 
factor, 𝑆𝑓 , that depends on both the major strain, r, and the through thickness, t.  At each 
time step the load curve is scaled by 𝑆𝑓  according to, 
𝑛+1
𝑆scaled load curve
= Sf(𝑟, 𝑡) × 𝑆load curve
, 
where the superscript denotes the time step.  The scale factor depends on r, which is a 
strain measure defined as,
𝑟 =
εmajorworkpiece
𝜀majorfld
. 
The scale factor, then, is given by, 
𝑆𝑓 =
⎧1
{{{
⎨
{{{
⎩
SFF
SFT
(1 − BIAS)×SFF +
𝑟 < FSL,   𝑡 < TSL
𝑟 > FSL,   𝑡 < TSL
𝑟 < FSL,   𝑡 > TSL
(1 + BIAS) × SFT 𝑟 > FSL,   𝑡 > TSL
Usually  SFF  is  slightly  less  than  unity  and  SFT  is  slightly  greater  than  unity  so  that 
𝑆load curve changes insignificantly from time step to time step.
*DEFINE 
Purpose:  This keyword allows for defining Forming Limit Diagram (FLD) using sheet 
metal thickness ‘t’ and strain hardening value ‘n’, applicable to shell elements only. 
This feature is available in LS-DYNA Revision 61435 and later releases. 
4 
5 
6 
7 
8 
  Card 1 
1 
Variable 
LCID 
Type 
I 
2 
TH 
F 
3 
TN 
F 
Default 
none 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
LCID 
Load curve ID. 
Sheet metal thickness. 
Strain hardening value of the sheet metal, as in power law (Swift).
TH 
TN 
Remarks: 
1.  This keyword is used  in conjunction with keyword *MAT_TRANSVERSELY_-
ANISOTROPIC_ELASTIC_PLASTIC_NLP_FAILURE,  and  for  shell  elements 
only.   For  detailed  formula  of  calculating  the  FLD  based  on  sheet metal  thick-
ness  and  n-value,  please  refer  to  the  following  paper:  Ming  F.    Shi,  Shawn  Ge-
lisse, “Issues on the AHSS Forming Limit Determination”, IDDRG 2006.  
2. 
3. 
It is noted that this FLD calculation method is limited to sheet metal steels with 
thickness  equal  to  or  less  than  2.5  mm,  and  it  is  not  suitable  for  aluminum 
sheets. 
In  a  validation  example  shown  in  Figure  15-15,  a  single  shell  element  is 
stretched  in  three  typical  strain  paths  (linear):  uniaxial,  plane  strain  and  equi-
biaxial.  Strain  limits  for  each  path  are  recovered  when  the  history  variable 
(Formability Index limit in *MAT_037) reaches 1.0, shown in Figure 15-16.  The 
top  most  point  (strain  limit)  of  each  strain  path  coincides  with  the  FLC  curve 
calculated according to the paper, indicating the FLC defined by this keyword 
is  working  correctly.    As  shown  in  a  partial  keyword  file  below,  the  FLC  is 
defined using a thickness value of 1.5 and n-value of 0.159.  The ‘LCID’ of 891 is
used  to  define  a  variable  ‘ICFLD’  in  keyword  *MAT_TRANSVERSELY_-
ANISOTROPIC_ELASTIC_PLASTIC_NLP_FAILURE. 
*MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLASTIC_NLP_FAILURE 
$      MID        RO         E        PR      SIGY      ETAN         R     
HLCID 
         1 7.830E-09 2.070E+05      0.28       0.0       0.0    -0.864       
200 
$      IDY        EA       COE     ICFLD 
                                     891 
*DEFINE_CURVE_FLC 
$ LCID, TH, TN 
891,1.5,0.159 
$ DP600 NUMISHEET'05 Xmbr, Power law fitted 
*DEFINE_CURVE 
200 
0.000,395.000 
0.001,425.200  
0.003,440.300  
... 
4.  For  aluminum  sheets,  *DEFINE_CURVE  can  be  used  to  input  the  FLC  for  the 
variable ‘ICFLD’ in *MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLAS-
TIC_NLP_FAILURE. 
x i a l
n i a
Plane strain
Equibiaxial
Shell
Unstrained
Figure 15-15.  A single shell strained in three different strain paths
Single Element Test
Uniaxial
Equi-biaxial
Plane Strain
Calculated FLC
 1
 0.8
 0.6
 0.4
 0.2
 0
-0.6
-0.4
-0.2
 0
 0.2
 0.4
Minor True Strain
Figure 15-16.  Validation of the FLC defined by this keyword
*DEFINE_CURVE_FUNCTION 
Purpose:    Define  a  curve  [for  example,  load  (ordinate  value)  versus  time  (abscissa 
value)] where the ordinate is given by a function expression.  The function can reference 
other  curve  definition,  kinematical  quantities,  forces,  interpolating  polynomials, 
intrinsic functions, and combinations thereof.  Please note that many functions require 
the definition of a local coordinate system .  To output the curve to 
an  ASCII  database,  see  *DATABASE_CURVOUT.    This  command  is  not  for  defining 
curves for material models.  Note that arguments appearing in square brackets “[ ]” are 
optional. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
SIDR 
Type 
I 
Default 
none 
I 
0 
Function Cards.  Insert as many cards as needed.  These cards are combined to form a 
single line of input.  The next keyword (“*”) card terminates this input.  
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Remarks 
VARIABLE 
LCID 
FUNCTION 
A80 
1 
DESCRIPTION 
Load curve ID.  Tables  and load curves may 
not share common ID's.  LS-DYNA allows load curve ID's and table 
ID's  to  be  used  interchangeably.    A  unique  number  has  to  be
defined.
VARIABLE 
DESCRIPTION 
SIDR 
Stress initialization by dynamic relaxation: 
EQ.0: load  curve  used  in  transient  analysis  only  or  for  other
applications, 
EQ.1: load  curve  used  in  stress  initialization  but  not  transient 
analysis, 
EQ.2: load  curve  applies  to  both  initialization  and  transient
analysis. 
FUNCTION 
Arithmetic  expression  involving  a  combination  of  the  following
possibilities. 
Constants and Variables: 
FUNCTION 
DESCRIPTION 
TIME 
Current simulation time 
TIMESTEP 
Current simulation time step 
PI 
DTOR 
RTOD 
Proportionality constant relating the circumference of a circle to its
diameter 
Degrees to radians conversion factor (𝜋/180) 
Radians to degrees conversion factor (180/𝜋) 
Intrinsic Functions: 
FUNCTION 
DESCRIPTION
ABS(𝑎) 
Absolute value of 𝑎 
AINT(𝑎) 
Nearest integer whose magnitude is not larger than a 
ANINT(𝑎) 
Nearest whole number to a 
MOD(𝑎1, 𝑎2) 
Remainder when 𝑎1 is divided by 𝑎2 
SIGN(𝑎1, 𝑎2) 
Transfer sign of 𝑎2 to magnitude of 𝑎1 
MAX(𝑎1, 𝑎2) 
Maximum of 𝑎1 and 𝑎2 
MIN(𝑎1, 𝑎2) 
Minimum of 𝑎1 and 𝑎2
*DEFINE_CURVE_FUNCTION 
DESCRIPTION
SQRT(𝑎) 
Square root of 𝑎 
EXP(𝑎) 
LOG(𝑎) 
𝑒 raised to the power of 𝑎 
Natural logarithm of 𝑎 
LOG10(𝑎) 
Log base 10 of 𝑎 
SIN(𝑎) 
COS(𝑎) 
Sine of 𝑎 
Cosine of 𝑎 
TAN(𝑎) 
Tangent of 𝑎 
ASIN(𝑎) 
Arc sine of 𝑎 
ACOS(𝑎) 
Arc cosine of 𝑎 
ATAN(𝑎) 
Arc tangent of 𝑎 
ATAN2(𝑎1, 𝑎2)  Arc tangent of 𝑎1/𝑎2 
SINH(𝑎) 
Hyperbolic sine of 𝑎 
COSH(𝑎) 
Hyperbolic cosine of 𝑎 
TANH(𝑎 ) 
Hyperbolic tangent of 𝑎 
Load Curves: 
FUNCTION 
LCn 
DESCRIPTION 
Ordinate  value  of  curve  n  defined  elsewhere
FUNCTION 
DESCRIPTION 
DELAY(LC𝑛, 𝑡delay, 𝑦def)  Delays  curve  𝑛,  defined  by  *DEFINE_CURVE_FUNC-
TION,  *DEFINE_FUNCTION  or  DEFINE_CURVE,  by 
Tdelay  when simulation time ≥ Tdelay, and sets  the delayed 
curve value to Ydef when time < Tdelay, i.e., 
𝑓delay(𝑡) =
{⎧ 𝑓 (t− 𝑡delay)
⎩{⎨
𝑦def
𝑡 ≥ 𝑡delay
𝑡 < 𝑡delay
For  a  nonlinear  curve,  a  Tdelay  equal  to  more  than  5,000 
time steps might compromise the accuracy and must be
used with caution.   
When  Tdelay  is  a  negative  integer,  delay  time  is  input  in 
terms  of  time  step.    |Tdelay|  is  the  number  of  delay  time 
steps.    In  such  case,  |Tdelay|  is  limited  to  a  maximum  of 
100.  For example, Tdelay = -2 delays the curve by 2 time 
steps. 
Coordinate Functions: 
FUNCTION 
DESCRIPTION 
CX(𝑛) 
CY(𝑛) 
CZ(𝑛) 
Value of 𝑥-coordinate for node 𝑛. 
Value of 𝑦-coordinate for node 𝑛. 
Value of 𝑧-coordinate for node 𝑛. 
Displacement Functions: 
FUNCTION 
DM(𝑛1[, 𝑛2]) 
DESCRIPTION
Magnitude  of  translational  displacement  of  node  𝑛1  relative  to 
node 𝑛2.  Node 𝑛2 is optional and if omitted the displacement is 
computed relative to ground. 
DMRB(𝑛) 
Magnitude of translational displacement of rigid body having a
part ID of 𝑛
DX(𝑛1[, 𝑛2, 𝑛3]) 
DY(𝑛1[, 𝑛2, 𝑛3]) 
DZ(𝑛1[, 𝑛2, 𝑛3]) 
DXRB(𝑛) 
DYRB(𝑛) 
DZRB(𝑛) 
AX(𝑛1[, 𝑛2]) 
AY(𝑛1[, 𝑛2]) 
AZ(𝑛1[, 𝑛2]) 
*DEFINE_CURVE_FUNCTION 
DESCRIPTION
𝑥-translational  displacement  of  node  𝑛1  relative  to  node  𝑛2
expressed  in  the  local  coordinate  system  of  node  𝑛3.    In  other 
words,  at  any  time  t,  the  function  returns  the  component  of
relative  displacement  that  lies  in  the  x-direction  of  the  local 
coordinate  system  at  time = t.    If  node  𝑛2  is  omitted  it  defaults 
to  ground.    If  node  𝑛3  is  not  specified  the  displacement  is 
reported in the global coordinate system. 
𝑦-translational  displacement  of  node  𝑛1  relative  to  node  𝑛2
expressed  in  the  local  coordinate  system  of  node  𝑛3.    In  other 
words,  at  any  time  t,  the  function  returns  the  component  of
relative  displacement  that  lies  in  the  y-direction  of  the  local 
coordinate  system  at  time = t.    If  node  𝑛2  is  omitted  it  defaults 
to  ground.    If  node  𝑛3  is  not  specified  the  displacement  is 
reported in the global coordinate system. 
𝑧-translational  displacement  of  node  𝑛1  relative  to  node  𝑛2
expressed  in  the  local  coordinate  system  of  node  𝑛3.    In  other 
words,  at  any  time  t,  the  function  returns  the  component  of
relative  displacement  that  lies  in  the  z-direction  of  the  local 
coordinate  system  at  time = t.    If  node  𝑛2  is  omitted  it  defaults 
to  ground.    If  node  𝑛3  is  not  specified  the  displacement  is 
reported in the global coordinate system. 
𝑥-translational displacement of rigid body having a part ID of 𝑛
𝑦-translational displacement of rigid body having a part ID of 𝑛
𝑧-translational displacement of rigid body having a part ID of 𝑛
Rotation  displacement  of  node  𝑛1  about  the  local  𝑥-axis  of 
node 𝑛2.    If  𝑛2  is  not  specified  then  it  defaults  to  ground.    In
computing this value it is assumed the rotation about the other
two axes (𝑦-, 𝑧-axes) of node 𝑛2 is zero. 
Rotation  displacement  of  node  𝑛1  about  the  local  𝑦-axis  of 
node 𝑛2 .    If  𝑛2  is  not  specified  then  it  defaults  to  ground.    In
computing this value it is assumed the rotation about the other
two axes (𝑥-, 𝑧-axes) of node 𝑛2 is zero.  See Remark 1. 
Rotation  displacement  of  node  𝑛1  about  the  local  𝑧-axis  of 
node 𝑛2.    If  𝑛2  is  not  specified  then  it  defaults  to  ground.    In
computing this value it is assumed the rotation about the other
two axes (𝑥-, 𝑦-axes) of node 𝑛2 is zero.  See Remark 1.
FUNCTION 
PSI(𝑛1[, 𝑛2]) 
DESCRIPTION
First  angle  in  the  body2:313  Euler  rotation  sequence  which 
orients  node  𝑛1  in  the  frame  of  node 𝑛2.    If  𝑛2  is  omitted  it 
defaults to ground.  See Remark 1. 
THETA(𝑛1[, 𝑛2]) 
Second  angle  in  the  body2:313  Euler  rotation  sequence  which
orients  node  𝑛1  in  the  frame  of  node 𝑛2.    If  𝑛2  is  omitted  it 
defaults to ground.  See Remark 1. 
PHI(𝑛1[, 𝑛2]) 
Third  angle  in  the  body2:313  Euler  rotation  sequence  which
orients  node  𝑛1  in  the  frame  of  node 𝑛2.    If  𝑛2  is  omitted  it 
defaults to ground.  See Remark 1. 
YAW(𝑛1[, 𝑛2]) 
First  angle  in  the  body3:321  yaw-pitch-roll  rotation  sequence 
which orients node 𝑛1 in the frame of node 𝑛2.  If 𝑛2 is omitted it 
defaults to ground.  See Remark 1. 
PITCH(𝑛1[, 𝑛2]) 
Second angle in the body3:321 yaw-pitch-roll rotation sequence 
which orients node 𝑛1 in the frame of node 𝑛2.  If 𝑛2 is omitted it 
defaults to ground.  See Remark 1. 
ROLL(𝑛1[, 𝑛2]) 
Third  angle  in  the  body3:321  yaw-pitch-roll  rotation  sequence 
which orients node 𝑛1 in the frame of node 𝑛2.  If 𝑛2 is omitted it 
defaults to ground.  See Remark 1. 
Velocity Functions: 
FUNCTION 
VM(𝑛1[, 𝑛2]) 
DESCRIPTION
Magnitude  of  translational  velocity  of  node  𝑛1  relative  to 
node 𝑛2.    Node  𝑛2  is  optional  and  if  omitted  the  velocity  is 
computed relative to ground. 
VR(𝑛1[, 𝑛2]) 
Relative radial translational velocity of node 𝑛1 relative to node. 
If node 𝑛2 is omitted it defaults to ground. 
VX(𝑛1[, 𝑛2, 𝑛3]) 
𝑥-component of the difference between the translational velocity
vectors of node 𝑛1 and node 𝑛2 in the local coordinate system of 
node 𝑛3.  If node 𝑛2 is omitted it defaults to ground.  Node 𝑛3 is 
optional  and  if  not  specified  the  global  coordinate  system  is
used.
VY(𝑛1[, 𝑛2, 𝑛3]) 
VZ(𝑛1[, 𝑛2, 𝑛3]) 
*DEFINE_CURVE_FUNCTION 
DESCRIPTION
𝑦-component of the difference between the translational velocity
vectors of node 𝑛1 and node 𝑛2 in the local coordinate system of 
node 𝑛3.  If node 𝑛2 is omitted it defaults to ground.  Node 𝑛3 is 
optional  and  if  not  specified  the  global  coordinate  system  is
used. 
𝑧-component of the difference between the translational velocity
vectors of node 𝑛1 and node 𝑛2 in the local coordinate system of 
node 𝑛3.  If node 𝑛2 is omitted it defaults to ground.  Node 𝑛3 is 
optional  and  if  not  specified  the  global  coordinate  system  is
used. 
WM(𝑛1[, 𝑛2]) 
Magnitude  of  angular  velocity  of  node  𝑛1  relative  to  node 𝑛2. 
Node  𝑛2  is  optional  and  if  omitted  the  angular  velocity  is
computed relative to ground. 
WX(𝑛1[, 𝑛2, 𝑛3]) 
WY(𝑛1[, 𝑛2, 𝑛3]) 
WZ(𝑛1[, 𝑛2, 𝑛3]) 
𝑥-component  of  the  difference  between  the  angular  velocity
vectors of node 𝑛1 and node 𝑛2 in the local coordinate system of 
node 𝑛3.  If node 𝑛2 is omitted it defaults to ground.  Node 𝑛3is 
optional  and  if  not  specified  the  global  coordinate  system  is
used.  See Remark 1. 
𝑦-component  of  the  difference  between  the  angular  velocity
vectors of node 𝑛1 and node 𝑛2in the local coordinate system of 
node 𝑛3.  If node 𝑛2 is omitted it defaults to ground.  Node 𝑛3is 
optional  and  if  not  specified  the  global  coordinate  system  is
used.  See Remark 1. 
𝑧-component  of  the  difference  between  the  angular  velocity
vectors of node 𝑛1 and node 𝑛2 in the local coordinate system of 
node 𝑛3.    If  node  𝑛2is  omitted  it  defaults  to  ground.    Node  𝑛3is 
optional  and  if  not  specified  the  global  coordinate  system  is
used.  See Remark 1. 
Acceleration Functions: 
FUNCTION 
ACCM(𝑛1[, 𝑛2]) 
DESCRIPTION
Magnitude of translational acceleration of node 𝑛1 relative to 
node 𝑛2.    Node 𝑛2 is  optional  and  if  omitted  the  acceleration 
is computed relative to ground.  See Remark 1.
FUNCTION 
ACCX(𝑛1[, 𝑛2, 𝑛3]) 
ACCY(𝑛1[, 𝑛2, 𝑛3]) 
ACCZ(𝑛1[, 𝑛2, 𝑛3]) 
DESCRIPTION
𝑥-component  of  the  difference  between  the  translational
acceleration  vectors  of  node  𝑛1  and  node  𝑛2 in  the  local 
coordinate  system  of  node 𝑛3.    If  node  𝑛2  is  omitted  it 
defaults  to  ground.    Node 𝑛3 is  optional  and  if  not  specified 
the global coordinate system is used.  See Remark 1. 
𝑦-component  of  the  difference  between  the  translational 
acceleration  vectors  of  node  𝑛1  and  node  𝑛2 in  the  local 
coordinate  system  of  node 𝑛3.    If  node  𝑛2 is  omitted  it 
defaults  to  ground.    Node  𝑛3is  optional  and  if  not  specified 
the global coordinate system is used.  See Remark 1. 
𝑧-component  of  the  difference  between  the  translational
acceleration  vectors  of  node  𝑛1 and  node  𝑛2 in  the  local 
coordinate  system  of  node 𝑛3.    If  node  𝑛2  is  omitted  it 
defaults  to  ground.    Node 𝑛3 is  optional  and  if  not  specified 
the global coordinate system is used.  See Remark 1. 
WDTM(𝑛1[, 𝑛2]) 
Magnitude  of  angular  acceleration  of  node  𝑛1  relative  to 
node 𝑛2.    Node  𝑛2  is  optional  and  if  omitted  the  angular 
acceleration is computed relative to ground.  See Remark 1. 
WDTX(𝑛1[, 𝑛2, 𝑛3]) 
WDTY(𝑛1[, 𝑛2, 𝑛3]) 
WDTZ(𝑛1[, 𝑛2, 𝑛3]) 
the  difference  between 
the  angular
𝑥-component  of 
acceleration  vectors  of  node  𝑛1  and  node  𝑛2  in  the  local 
coordinate  system  of  node 𝑛3.    If  node  𝑛2  is  omitted  it 
defaults  to  ground.    Node 𝑛3  is  optional  and  if  not  specified 
the global coordinate system is used.  See Remark 1. 
the  difference  between 
𝑦-component  of 
the  angular 
acceleration  vectors  of  node  𝑛1and  node  𝑛2  in  the  local 
coordinate  system  of  node 𝑛3.    If  node  𝑛2  is  omitted  it 
defaults  to  ground.    Node 𝑛3  is  optional  and  if  not  specified 
the global coordinate system is used.  See Remark 1. 
the  difference  between 
𝑧-component  of 
the  angular
acceleration  vectors  of  node  𝑛1  and  node  𝑛2  in  the  local 
coordinate  system  of  node 𝑛3.    If  node  𝑛2 is  omitted  it 
defaults  to  ground.    Node 𝑛3  is  optional  and  if  not  specified 
the global coordinate system is used.  See Remark 1.
*DEFINE_CURVE_FUNCTION 
FUNCTION 
FM(𝑛1[, 𝑛2]) 
FX(𝑛1[, 𝑛2, 𝑛3]) 
FY(𝑛1[, 𝑛2, 𝑛3]) 
FZ(𝑛1[, 𝑛2, 𝑛3]) 
DESCRIPTION
Magnitude  of  the  SPC  force  acting  on  node  𝑛1  minus  the  force 
acting  on  node 𝑛2.    Node  𝑛2  is  optional  and  if  omitted  the  force 
that acting only on 𝑛1 Is returned.  See Remark 1. 
𝑥-component of SPC force acting on node 𝑛1 as computed in the 
optional  local  system  of  node 𝑛3.    If  𝑛2  is  specified,  the  force 
acting  on  𝑛2  is  subtracted  from  the  force  acting  on 𝑛1.    See 
Remark 1. 
𝑦-component of SPC force acting on node 𝑛1 as computed in the 
optional  local  system  of  node 𝑛3.    If  𝑛2  is  specified,  the  force 
acting  on  𝑛2  is  subtracted  from  the  force  acting  on 𝑛1.    See 
Remark 1. 
𝑧-component of SPC force acting on node 𝑛1 as computed in the 
optional  local  system  of  node 𝑛3.    If  𝑛2  is  specified,  the  force 
acting  on  𝑛2  is  subtracted  from  the  force  acting  on 𝑛1.    See 
Remark 1. 
TM(𝑛1[, 𝑛2]) 
Magnitude  of  SPC  torque  acting  on  node  𝑛1  minus  the  torque 
acting node 𝑛2.  Node 𝑛2 is optional and if omitted the torque that 
acting only on 𝑛1.  See Remark 1. 
TX(𝑛1[, 𝑛2, 𝑛3]) 
TY(𝑛1[, 𝑛2, 𝑛3]) 
TZ(𝑛1[, 𝑛2, 𝑛3]) 
𝑥-component of the SPC torque acting on node 𝑛1 as computed in 
the optional local system of node 𝑛3.  If 𝑛2 is specified, the torque 
acting  on  𝑛2  is  subtracted  from  the  torque  acting  on 𝑛1.    See 
Remark 1. 
𝑦-component of the SPC torque acting on node 𝑛1 as computed in 
the optional local system of node 𝑛3.  If 𝑛2 is specified, the torque 
acting  on  𝑛2  is  subtracted  from  the  torque  acting  on 𝑛1.    See 
Remark 1. 
𝑧-component of the SPC torque acting on node 𝑛1 as computed in 
the optional local system of node 𝑛3.  If 𝑛2 is specified, the torque 
acting  on  𝑛2  is  subtracted  from  the  torque  acting  on 𝑛1.    See 
Remark 1.
Sensor Functions: 
FUNCTION 
SENSOR(𝑛) 
DESCRIPTION
Returns a value of 1.0 if *SENSOR_CONTROL of control ID 𝑛
has  a  status  of  “on”.    If  the  sensor  has  a  status  of  “off”,  then
the returned value is equal to the value of the TYPEID field on 
to
*SENSOR_CONTROL  when 
“function,” otherwise SENSOR(𝑛) returns zero. 
the  TYPE 
is  set 
field 
SENSORD(𝑛, 𝑖𝑑𝑓𝑙𝑡) 
Returns the current value of *SENSOR_DEFINE sensor having 
ID  𝑛.    Idflt  is  the  optional  filter  ID  defined  using  *DEFINE_-
FILTER. 
Contact Force Functions: 
FUNCTION 
DESCRIPTION 
RCFORC(id, ims, comp, local) 
Returns the component comp  
of  contact  interface  id    as 
calculated  in  the  local  coordinate  system  local  .    If  local  equals  zero 
then  forces  are  reported  in  the  global  coordinate
system.  Forces are reported for the slave side when 
ims = 1 or master side when ims = 2. 
Following  are  the  admissible  values  of  comp  and 
their corresponding force component. 
comp.EQ.1: 𝑥 force component 
comp.EQ.2: 𝑦 force component 
comp.EQ.3: 𝑧 force component 
comp.EQ.4: resultant force 
Element Specific Functions: 
FUNCTION 
DESCRIPTION 
BEAM(id, jflag, comp, rm) 
the 
comp 
force  component 
Returns 
  of  beam  id  as  calculated  in
the  local  coordinate  system  rm.    Forces  are
reported in the global coordinate system if rm is
zero.    If  rm  equals  -1  the  beam’s  𝑟,  𝑠,  and  𝑡
force/moment is returned.  If jflag is set to zero
FUNCTION 
DESCRIPTION 
then  the  force/torque  acting  on  𝑛1  end  of  the
beam is returned, otherwise if jflag is set to 1 the
force/torque  on  the  𝑛2  end  of  the  beam  is
returned.  See *ELEMENT_BEAM for the nodal
connectivity rule defining 𝑛1 and 𝑛2. 
Admissible  values  of  comp  are  1-8  and
correspond to the following components. 
comp.EQ.1: force magnitude 
comp.EQ.2: 𝑥 force (axial 𝑟-force, rm = -1) 
comp.EQ.3: 𝑦 force (𝑠-shear force, rm = -1) 
comp.EQ.4: 𝑧 force (𝑡-shear force, rm = -1) 
comp.EQ.5: torque magnitude 
comp.EQ.6: 𝑥 torque  (torsion, rm = -1) 
comp.EQ.7: 𝑦 torque (𝑠-moment, rm = -1) 
comp.EQ.8: 𝑧 torque (𝑡-moment, rm = -1) 
ELHIST(eid, etype, comp, ipt, local) 
the  elemental  quantity  comp 
Returns 
  of  element  eid  as  calculated
in  the  local  coordinate  system  local.    Quantities
are  reported  in  the  global  coordinate  system  if
  The  parameter  ipt  specifies
local  is  zero. 
for  particular
whether 
integration  point  or  maximum,  minimum,  or
averaging  is  applied  across  the  integration
points. 
the  quantity 
is 
The  following  element  classes,  specified  with
etype, are supported. 
etype.EQ.0:  solid 
etype.EQ.2: 
thin shell 
Following are admissible values of comp and the
corresponding elemental quantity. 
comp.EQ.1:  𝑥 stress 
comp.EQ.2:  𝑦 stress 
comp.EQ.3:  𝑧 stress 
comp.EQ.4:  𝑥𝑦 stress
FUNCTION 
DESCRIPTION 
comp.EQ.5: 𝑦𝑧 stress 
comp.EQ.6:  𝑧𝑥 stress 
comp.EQ.7:  effective plastic strain 
comp.EQ.8:  hydrostatic pressure 
comp.EQ.9:  effective stress 
comp.EQ.11: 𝑥 strain 
comp.EQ.12: 𝑦 strain 
comp.EQ.13: 𝑧 strain 
comp.EQ.14: 𝑥𝑦 strain 
comp.EQ.15: 𝑦𝑧 strain 
comp.EQ.16: 𝑧𝑥 strain 
Integration  point  options,  specified  with  ipt,
follow. 
ipt.GE.1:  quantity is reported for integration
point number ipt 
ipt.EQ.-1:  maximum  of  all  integration  points
(default) 
ipt.EQ.-2:  average of all integration points 
ipt.EQ.-3:  minimum of all integration points 
ipt.EQ.-4:  lower surface integration point 
ipt.EQ.-5:  upper surface integration point 
ipt.EQ.-6:  middle surface integration point 
local  currently
The  local  coordinate  option 
defaults  to  the  global  coordinate  system  for
solid  elements  and  other  coordinate  system
options are unavailable.  In the case of thin shell
elements  the  quantity  is  reported  only  in  the
element local coordinate system. 
local.EQ.1:  global  coordinate  system  (solid
elements) 
local.EQ.2:  element  coordinate  system  (thin
shell elements)
FUNCTION 
DESCRIPTION 
JOINT(id, jflag, comp, rm) 
the 
comp 
force  component 
Returns 
 due to rigid body joint id as
calculated in the local coordinate system rm.  If
jflag  is  set  to  zero  then  the  force/torque  acting
on  𝑛1  end  of  the 
  The
force/torque  on  the  𝑛2  end  of  the  joint  is
returned  if 
  See  *CON-
jflag  is  set  to  1. 
STRAINED_JOINT for the rule defining n1 and
𝑛2.  
joint  is  returned. 
Admissible  values  of  comp  are  1-8  and
correspond to the following components. 
comp.EQ.1: force magnitude 
comp.EQ.2: 𝑥 force 
comp.EQ.3: 𝑦 force 
comp.EQ.4: 𝑧 force 
comp.EQ.5: torque magnitude 
comp.EQ.6: 𝑥 torque 
comp.EQ.7: 𝑦 torque 
comp.EQ.8: 𝑧 torque 
Nodal  Specific Functions: 
FUNCTION 
DESCRIPTION
TEMP(𝑛) 
Returns the temperature of node 𝑛 
General Functions 
FUNCTION 
DESCRIPTION 
CHEBY(𝑥, 𝑥0, 𝑎0, … , 𝑎30) 
Evaluates  a  Chebyshev  polynomial  at  the  user
specified value 𝑥.  The parameters 𝑥0, 𝑎0, 𝑎1, …, 𝑎30
are  used 
the
to  define 
polynomial defined by: 
the  constants 
for 
𝐶(𝑥) = ∑ 𝑎𝑗𝑇𝑗(𝑥 − 𝑥0) 
where the functions 𝑇𝑗 is defined recursively as
FUNCTION 
DESCRIPTION 
𝑇𝑗(𝑥 − 𝑥0) = 2(𝑥 − 𝑥0)𝑇𝑗−1(𝑥 − 𝑥0) − 𝑇𝑗−2(𝑥 − 𝑥0)
where 
𝑇0(𝑥 − 𝑥0) = 1 
𝑇1(𝑥 − 𝑥0) = 𝑥 − 𝑥0 
Evaluates  a  Fourier  cosine  series  at  the  user
specified  value  x.    The  parameters  x0,  a0,  a1,  …, 
a30 are used to define the constants for the  series
defined by: 
𝐹(𝑥) = ∑ 𝑎𝑗𝑇𝑗(𝑥 − 𝑥0) 
where 
𝑇𝑗(𝑥 − 𝑥0) = cos[𝑗ω(𝑥 − 𝑥0)] 
Evaluates  a  Fourier  sine  series  at  the  user
specified value 𝑥.  The parameters 𝑥0, 𝑎0, 𝑎1, …, 𝑎30
are  used  to  define  the  constants  for  the  series
defined by: 
𝐹(𝑥) = ∑ 𝑎𝑗𝑇𝑗(𝑥 − 𝑥0) 
where 
𝑇𝑗(𝑥 − 𝑥0) = sin[𝑗ω(𝑥 − 𝑥0)] 
Arithmetic  if  conditional  where  𝑎𝑖  can  be  a 
constant or any legal expression described in *DE-
FINE_CURVE_FUNCTION. 
example, 
𝑎1=’CX(100)’  sets  the  first  argument  to  be  the  x-
coordinate of node 100.  
{⎧the value of  𝑎2
the value of  𝑎3
⎩{⎨
the value of  𝑎4
if the value of 𝑎1 < 0
if the value of 𝑎1 = 0
if the value of 𝑎1 > 0
IF =
For 
Evaluates the control signal of a PID controller 
d𝑒(𝑡)
d𝑡
𝑢(𝑡) = kp× 𝑒(𝑡) + ki× ∫ 𝑒(𝜏)𝑑𝜏
+ kd×
FORCOS(𝑥, 𝑥0, 𝜔[, 𝑎0, … , 𝑎30]) 
FORSIN(𝑥, 𝑥0, 𝜔[, 𝑎0, … , 𝑎30]) 
IF(𝑎1, 𝑎2, 𝑎3, 𝑎4) 
PIDCTL(meas, ref, kp, ki, kd,  tf, 
ei0, sint, umin, umax) 
where  𝑒(𝑡)  is  the  control  error  defined  as  the 
difference between the reference value ref and the 
measured value, meas 
𝑒(𝑡) = ref− 𝑚𝑒𝑎𝑠
FUNCTION 
DESCRIPTION 
The  control  parameters  are  proportional  gain  kp, 
integral  gain  ki,  derivative  gain  kd  and  low-pass 
filter tf for the derivative calculation 
d𝑒(𝑡𝑛)
d𝑡
=
d𝑒(𝑡𝑛−1)
d𝑡
𝑡𝑓
∆𝑡 + 𝑡𝑓
+
∆𝑡
∆𝑡 + 𝑡𝑓
×
𝑒(𝑡𝑛) − 𝑒(𝑡𝑛−1)
∆𝑡
Ei0 is the initial integral value at time = 0.  
Sint is the sampling interval.  Umin and umax, the 
lower  and  upper  limit  of  a  control  signal,  can  be
used  to  represent  the  saturation  limits  of  an
actuator.  When the signal is not within the limits,
it is clipped to the saturation limit, i.e., integration
is skipped to avoid integrator wind-up. 
Input  parameter  can  be  a  constant  or  any  legal
*DEFINE_CURVE_-
expression  described 
  For  example,  meas=’CX(100)’
FUNCTION. 
measures  the  x-coordinate  of  node  100,  ref
=’LC200’ uses curve 200 as the reference value. 
in 
POLY(𝑥, 𝑥0, 𝑎0, … , 𝑎30) 
SHF(𝑥, 𝑥0, 𝑎, 𝜔[, 𝜙, 𝑏]) 
Evaluates  a  standard  polynomial  at  the  user
specified value 𝑥.  The parameters 𝑥0, 𝑎0, 𝑎1, …, 𝑎30
the
to  define 
are  used 
polynomial defined by: 
the  constants 
for 
𝑃(𝑥) = 𝑎0 + 𝑎1(𝑥 − 𝑥0) + 𝑎2(𝑥 − 𝑥0)2
+ ⋯ + 𝑎𝑛(𝑥 − 𝑥0)𝑛
Evaluates  a  Fourier  sine  series  at  the  user
specified value 𝑥.  The parameters 𝑥0, 𝑎0, 𝑎1, …, 𝑎30
are  used  to  define  the  constants  for  the  series
defined by: 
SHF = 𝑎sin[ω(𝑥 − 𝑥0) − ϕ] + 𝑏 
STEP(𝑥, 𝑥0, ℎ0, 𝑥1, ℎ1) 
Approximates the Heaviside function with a cubic 
polynomial using the equation: 
STEP =
⎧ℎ0
{
{
⎨
{
{
⎩
ℎ1
ℎ0 + (ℎ1 − ℎ0) [
(𝑥 − 𝑥0)
]
(𝑥1 − 𝑥0)
{3 − 2 [
(𝑥 − 𝑥0)
(𝑥1 − 𝑥0)
if 𝑥 ≤ 𝑥0
]} if 𝑥 < 𝑥 < 𝑥1
if 𝑥 ≥ 𝑥1
Electromagnetic solver (EM) Functions 
FUNCTION 
DESCRIPTION 
EM_ELHIST(iele, ifield, idir) 
Returns  the  elemental  quantity  of  element  iele  in 
the global reference frame. 
EM_NDHIST(inode, ifield, idir) 
RM_PAHIST(ipart, ifield, idir) 
Returns  the  nodal  quantity  of  node  inode  in  the 
global reference frame. 
Returns  the  value  integrated  over  the  whole  part 
given by ipart. ifield can be 7, 8 and 11 only. 
Admissible values of ifield are 1-10 and correspond 
to the following variables. 
comp.EQ.1:  scalar potential 
comp.EQ.2:  vector potential 
comp.EQ.3:  electric field 
comp.EQ.4:  𝐁 field 
comp.EQ.5:  𝐇 field 
comp.EQ.6:  current density 
comp.EQ.7:  Lorentz force 
comp.EQ.8:  current density 
comp.EQ.9:  Lorentz force 
comp.EQ.10: relative permeability 
comp.EQ.11: magnetic energy (in the conductor 
only) 
Admissible values of idir are 1-4 and correspond to 
the following components. 
comp.EQ.1: 𝑥-component 
comp.EQ.2: 𝑦-component 
comp.EQ.3: 𝑧-component 
comp.EQ.4: Norm 
Remarks: 
1.  Local  Coordinate  Systems  Required  for  Rotational  Motion.    A  local 
coordinate system must be attached to nodes if they are referenced by functions
involving  rotational  motion,  for  example,  angular  displacement  or  angular 
velocity.  The local coordinate system is attached to the node using *DEFINE_-
COORDINATE_NODES and FLAG=1 is a requirement.  Furthermore, the three 
nodes which comprise the coordinate system must lie on the same body.  Simi-
larly, a local coordinate system must also be attached to node 𝑛3 if 𝑛3 is refer-
enced  in  functions:  DX,  DY,  DZ,  VX,  VY,  VZ,  WX,  WY,  WZ,  ACCX,  ACCY, 
ACCZ, WDTX, WDTY, WDTZ, FX, FY, FZ, TX, TY, or TZ. 
2.  Default is Radians.   Unless otherwise noted units of radians are  always used 
for the arguments and output of functions involving angular measures. 
3.  The following examples serve only as an illustration of syntax. 
Example 1: 
Define a curve 10 whose ordinate is, 
𝑓 (𝑥) =
(ordinate of load curve 9) × (magnitude of translation velocity at node 22)3. 
*DEFINE_CURVE_FUNCTION 
10 
0.5*lc9*vm(22)**3 
Example 2: 
Define a curve 101 whose ordinate is, 
𝑓 (𝑥) = −2(z translational displacement of node 38) × sin(20𝜋𝑡). 
*DEFINE_CURVE_FUNCTION 
101 
-2.*dz(38)*sin(2.*pi*10.*time) 
Example 3: 
Define a curve 202 whose ordinate is, 
𝑓 (𝑥) = {
cos(4𝜋𝑡) 𝑖𝑓  𝑡 ≤ 5.
0. 𝑖𝑓  𝑡  > 5.
*DEFINE_CURVE_FUNCTION 
202 
If(TIME-5.,COS(4.*PI*TIME),COS(4.*PI*TIME),0.)
*DEFINE 
Purpose:  Define a smoothly varying curve using few parameters.  This shape is useful 
for velocity control of tools in metal forming applications. 
Vmax
Trise
Trise
dist = ∫v(t)dt
0.0
0.0
Tstart
Simulation Time
Tend
Figure 15-17.  Smooth curve created automatically using *DEFINE_CURVE_-
SMOOTH.  This shape is commonly used to control velocity of tools in metal
forming applications as shown in the  above  graph, but  can  be used  for other
applications in place of any standard load curve. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
SIDR 
DIST 
TSTART 
TEND 
TRISE 
VMAX 
Type 
I 
I 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
LCID 
Load curve ID, must be unique.
*DEFINE_CURVE_SMOOTH 
DESCRIPTION
SIDR 
Stress initialization by dynamic relaxation: 
EQ.0: load  curve  used  in  transient  analysis  only  or  for  other 
applications, 
EQ.1: load  curve  used  in  stress  initialization  but  not  transient
analysis, 
EQ.2: load  curve  applies  to  both  initialization  and  transient
analysis. 
DIST 
Total distance tool will travel (area under curve). 
TSTART 
Time curve starts to rise 
TEND 
Time  curve  returns  to  zero.    If  TEND  is  nonzero,  VMAX  will  be
computed  automatically  to  satisfy  required  travel  distance  DIST.
Input either TEND or VMAX. 
TRISE 
Rise time 
VMAX 
Maximum  velocity  (maximum  value  of  curve).    If  VMAX  is
nonzero,  TEND  will  be  computed  automatically  to  satisfy
required travel distance DIST.  Input either TEND or VMAX.
*DEFINE_CURVE_TRIM_{OPTION} 
Available options include: 
<BLANK> 
3D 
NEW 
Purpose:    This  keyword  is  developed  to  define  curves  and  controls  for  sheet  blank 
trimming in sheet metal forming.  It can also be used to define mesh adaptivity along a 
curve  prior  to  the  start  of  a  simulation,  using  variable  TCTOL  and  keyword  *CON-
TROL_ADAPTIVE_CURVE. 
When  the  option  3D  is  used,  the  trimming  is  processed  based  on  the  element  normal 
rather than a vector.  The option NEW is used to trim in a fixed direction specified by a 
vector, and is also called 2D trimming.  Currently this keyword applies to: 
•  2D and 3D trimming of shell elements, 
•  2D and 3D trimming of solids, 
•  2D and 3D adaptive trimming of adaptive-meshed sandwiched parts (limit to a 
core  of  one  layer  of  solid  elements  with  outer  layers  of  shell  elements,  see 
“IFSAND” under *CONTROL_ADAPTIVE), 
•  2D and 3D trimming of non-adaptive sandwiched parts (a core of multiple layers 
of solid elements with outer layers of shell elements), and, 
•  2D trimming of thick shell elements (TSHELL). 
This  keyword  is  not  applicable  to  axisymmetric  solids  or  2D  plane  strain/stress 
elements.    Related  keywords  include  *ELEMENT_TRIM,  *CONTROL_FORMING_-
TRIMMING,  *CONTROL_ADAPTIVE_CURVE,  *INCLUDE_TRIM,  and  *INCLUDE.  
Another  closely  related  keyword  is  *CONTROL_FORMING_TRIM_MERGE,  which 
automatically closes an open trim curve with a user-specified tolerance. 
Trimming  of  shell  and  solid  elements  are  supported  starting  in  LS-PrePost  4.0  and 
LS-PrePost 4.3, respectively, under Application → MetalForming → Easy Setup.
Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TCID 
TCTYPE 
TFLG 
TDIR 
TCTOL 
TOLN / 
IGB 
NSEED1  NSEED2 
Type 
I 
Default 
none 
I 
1 
I 
none 
I 
0 
F 
F 
I 
I 
0.25 
2.0 / 0 
none 
none 
Remarks 
Fig. 
15-18 
Fig. 
15-19 
Point Cards.  Additional cards for TCTYPE = 1.  Put one point per card (2E20.0).  Input 
is terminated at the next keyword (“*”) card.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
CX 
F 
Default 
0.0 
CY 
F 
0.0 
CZ 
F 
0.0 
IGES File Card.  Additional card for TCTYPE = 2.  
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
FILENAME 
C 
  VARIABLE   
DESCRIPTION
TCID 
ID number for trim curve.
VARIABLE   
DESCRIPTION
TCTYPE 
Trim curve type: 
EQ.1: Curve  data 
in  XYZ 
following
procedures  outlined  in  Figures  under  *INTERFACE_-
BLANKSIZE.  In addition, only this format is allowed in
*INTERFACE_COMPENSATION_NEW.  
format,  obtained 
EQ.2: IGES trim curve. 
TFLG 
Element removal option (applies to option NEW only): 
EQ.-1:  remove material outside curve; 
EQ.1:  remove material inside curve. 
TDIR 
If  the  option NEW  is  used,  this  is  the  ID  of  a  vector  (*DEFINE_-
VECTOR) giving the trim direction . 
EQ.0:  default  vector  (0.0,0.0,1.0)  is  used.    Curve  is  defined  in
global  XY  plane,  and  projected  onto  mesh  in  global  Z-
direction to define trim line. 
If the option 3D is used, TDIR is used to indicate whether the trim
curve is near the top or bottom surface of the solids or laminates
(>Revision 101964), see Trimming. 
EQ.1:  trim curve is located near the top surface (default). 
EQ.-1:  trim curve is located near the bottom surface. 
TCTOL 
Tolerance limiting size of small elements created during trimming
. 
LT.0:  "simple" trimming, producing jagged edge mesh 
When  used  together with  *CONTROL_ADAPTIVE_CURVE,  it  is 
a  distance  from  the  curve  out  (both  sides).    Within  this  distance
the blank mesh will be refined, as stated in remarks below.
TOLN / IGB 
*DEFINE_CURVE_TRIM 
DESCRIPTION
If  the  option  3D  is  used,  TOLN  represents  the  maximum  gap
between  the  trimming  curve  and  the  mesh.    If  the  gap  is  bigger 
than this value, this section in the curve will not be used.  
If  the  option  NEW  is  used,  then  the  variable  IGB  is  defined  as 
follows: 
IGB.EQ.0: trimming  curve  is  defined  in  local  coordinate
system.    This  is  the  default  value.    If  this  value  is
chosen for IGB, then the variable TDIR and the key-
word *DEFINE_VECTOR need to be defined accord-
ing to Figure 15-18. 
IGB.EQ.1: trimming  curve  is  defined  in  global  coordinate
system. 
NSEED1/ 
NSEED2 
A  node  ID  on  the  blank  in  the  area  that  remains  after  trimming,
applicable to both options 3D or NEW. 
LT.0: positive number is a node ID, which may not necessarily
be from the blank, referring to remarks below. 
CX, CY, CZ 
X,  Y,  Z-coordinate  of  trim  curve. 
TCTYPE = 1. 
  Define  if  and  only  if
FILENAME 
Name  of  IGES  database  containing  trim  curve(s).    Define  if  and
only if TCTYPE = 2. 
Trimming capability summary: 
This keyword and its options deal with trimming of the following scenarios: 
2D (along 
one 
direction) 
3D 
(element 
normal) 
2D & 3D 
Double 
Trim 
Adaptive mesh 
Shell 
Solids 
Yes 
Yes 
Yes 
Yes 
Yes 
Yes 
Yes 
N/A 
Laminates 
Yes 
Yes 
Yes 
One layer of 
solids only; 
Multiple layers of 
solids okay for 
non-adaptive 
mesh.
TSHELL 
Yes 
N/A 
N/A 
N/A 
About the options and trim curves: 
The  option  NEW  activates  a  new  searching  algorithm,  which  enables  a  much  faster 
trimming  operation  compared  with  option  3D.    For  big  models,  the  improvement  in 
computational  efficiency  of  the  NEW  option  is  significant.    In  addition,  users  are 
required to pick a seed node (or position coordinates), as is the case with the 3D option.  
Both  options  are  now  available  under  the  “Trimming”  feature  of  LS-PrePost  4.0’s  eZ-
Setup  for  metal  forming  application  (http://ftp.lstc.com/anonymous/outgoing/-
lsprepost/4.0/metalforming/).    Only  IGES  entities  110  and  106  are  supported  when 
using the TCTYPE of 2.  The eZ-Setup for trimming function ensures correct IGES files 
are written for trimming simulation. 
For the option NEW, Revision 68643 and later releases enable trimming of a part where 
trim lines go beyond the part boundary.  This is illustrated in Figure 15-24. 
Enclosed  trimming  curves  (same  start  and  end  points)  are  required  for  all  options.  
Furthermore,  for  each  enclosed  trimming  curve,  only  one  curve  segment  is  acceptable 
for  the  option  3D;  while  several  curve  segments  are  acceptable  with  the  option  NEW.  
Curves can be manipulated through the use of Merge and break features in LS-PrePost4.0, 
found under Curve/Merge (always select piecewise under Merge) and break. 
In case of 3D trimming, trim curves need to be sufficiently close to the part.  A feature 
of  curve  projection  to  the  mesh  in  LS-PrePost  can  be  used  to  process  the  trim  curves.  
The  feature  is  accessible  under  GeoTol/Project/Closest  Proj/Project  to  Element/By  Part.  
Double precision LS-DYNA executable may also help in this situation. 
Choice  of  2D  or  3D  trimming  depends  on  the  to-be-trimmed  part  geometry.    2D 
trimming  can  be  used  if  trimming  is  to  be  done  on  the  relatively  flat  area  of  the  part, 
while  3D  trimming  must  be  selected  for  trimming  on  a  inclined  or  vertical  draw  wall 
area for precise trimming. 
Seed node definition: 
This keyword in combination with *ELEMENT_TRIM trims the requested parts before a 
job starts (pre-trimming), and can handle adaptive mesh.  If the keyword *ELEMENT_-
TRIM does not exist the parts are trimmed after the job is terminated (post-trimming). 
Seed node is used to define which side of the drawn panel to be kept after the trimming.  
With  the  frequent  application  of  adaptive  re-meshing,  the  seed  node  for  trimming  is 
often unknown until the draw forming is complete.  With the negative NSEED variable,
an  extra  node  unrelated  to  the  blank  and  tools  can  be  created  for  the  definition  of  the 
seed node, enabling trimming process independent of the previous process simulation 
results.    The  extra  node  can  be  defined  using  keyword  *NODE.    A  partial  keyword 
input example for the trimming of a double-attached NUMISHEET2002 fender outer with 
the  option  NEW  is  listed  below,  where  a  2D  trimming  is  performed  with  IGES  file 
doubletrim.iges  in  the  global  Z-axis,  with  two  nodes  of  negative  ID  43356  and  18764 
assigned to the variables NSEED1 and NSEED2, respectively.  The two seed nodes are 
defined  off  the  stationary  lower  post,  and  do  not  necessarily  need  to  be  a  part  of  the 
post,  as  shown  in Figure  15-20.    The  drawn  panels  in  wire  frame  are  shown  in Figure 
15-21,  along  with  the  thickness/thinning  contour  (Figure  15-22).    In  Figure  15-23,  the 
drawn panels are trimmed and separated. 
*KEYWORD 
*CONTROL_TERMINATION 
0.000 
*CONTROL_SHELL 
...... 
*CONTROL_OUTPUT 
...... 
*DATABASE_BINARY_D3PLOT 
...... 
*DATABASE_EXTENT_BINARY 
...... 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*SET_PART_LIST 
...... 
*PART 
Blank                                                                            
...... 
*SECTION_SHELL 
...... 
*MAT_3-PARAMETER_BARLAT 
...... 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*INCLUDE_TRIM 
drawn.dynain 
*ELEMENT_TRIM 
         1 
*DEFINE_CURVE_TRIM_NEW 
$#    TCID    TCTYPE      TFLG      TDIR     TCTOL      TOLN    NSEED1    NSEED2 
         1         2                   0     0.250         1    -43356    -18764 
doubletrim.iges 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*NODE 
18764,-184.565,84.755,78.392 
43356,-1038.41,119.154,78.375 
*INTERFACE_SPRINGBACK_LSDYNA 
...... 
*END 
If the seed node is too far away from the blank it will be projected to the blank and the 
new position will be used as the seed node.  Typically, this node can be selected from 
the stationary tool in its home position. 
Alternatively,  if  the  variable  NSEEDs  are  not  defined,  the  seeds  can  be  defined  using 
*DEFINE_TRIM_SEED_POINT_COORDINATES.  A partial keyword input is provided 
below for trimming of the same double-attached fender outer.
*INCLUDE_TRIM 
drawn.dynain 
*ELEMENT_TRIM 
         1 
*DEFINE_CURVE_TRIM_NEW 
$#    TCID    TCTYPE      TFLG      TDIR     TCTOL      TOLN    NSEED1    NSEED2 
         1         2                   0     0.250         1       
doubletrim.iges 
*DEFINE_TRIM_SEED_POINT_COORDINATES 
$    NSEED        X1        Y1        Z1        X2        Y2        Z2 
         2  -184.565    84.755    78.392  -1038.41   119.154    78.375 
Again,  selecting  a  seed  node  is  quite  easy  in  “Trimming”  process  of  LS-PrePost4.0 
eZSetup for metal forming application. 
General adaptive re-meshing and element fixing during trimming: 
In case of large element size along the trim curves, the blank mesh can be pre-adapted 
along  the  trim  curves  before  trimming  by  adding  the  keyword  *CONTROL_ADAP-
TIVE_CURVE  to  the  above  example  for  a  better  quality  trim  edge.    The  following 
indicates  refining  meshes  for  part  set  ID  1  no  more  than  three  levels  along  the  trim 
curves,  or  until  element  size  reaches  3.0:  Care  should  be  taken  since  too  small  of  the 
value SMIN and too large value of N could result in excessive amount of elements to be 
generated. 
*CONTROL_ADAPTIVE_CURVE 
$#   IDSET     ITYPE         N      SMIN   ITRIOPT 
         1         2         3       3.0         0 
Sometimes it is helpful to conduct a check of the trimmed mesh along the edge in the 
same  trimming  input  deck  using  the  keyword  *CONTROL_CHECK_SHELL.    This  is 
especially  useful  for  the  next  continued  process  simulation.    For detailed  usage,  check 
for an updated remarks for the keyword. 
The  trimming  tolerance  TCTOL  limits  the  size  of  the  smallest  element  created  during 
trimming.  A value of 0.0 places no limit on element size.  A value of 0.5 restricts new 
elements to be at least half of the size of the parent element.  A value of 1.0 allows no 
new  elements  to  be  generated,  only  repositioning  of  existing  nodes  to  lie  on  the  trim 
curve.    A  negative  tolerance  value  activates  "simple"  trimming,  where  entire  elements 
are removed, leaving a jagged edge. 
TCTOL used as mesh refinement width along a curve: 
The  variable  TCTOL  can  be  used  to  control  the  mesh  refinement  along  a  curve  when 
used together with *CONTROL_ADAPTIVE_CURVE.  In this scenario, it is the distance 
from both sides of the curve within which the mesh will be refined.  The mesh will be 
refined  in  the  beginning  of  the  simulation.    This  method  offers  greater  control  on  the 
number  of  elements  to  be  generated  during  mesh  refinement,  as  compared  to  that 
without using this variable.  A detailed description and example is provided under the 
manual section under *CONTROL_ADAPTIVE_CURVE.
The  keyword  *INCLUDE_TRIM  is  recommended  to  be  used  at  all  times,  either  for 
trimming  or  for  mesh  refinement  purpose,  except  in  case  where  to-be-trimmed  sheet 
blank  has  no  stress  and  strain  information  (no  *INITIAL_STRESS_SHELL,  and  *INI-
TIAL_STRAIN_SHELL  cards  present  in  the  sheet  blank  keyword  or  dynain  file),  the 
keyword  *INCLUDE  must  be  used.    A  check  box  to  indicate  that  the  blank  is  free  of 
stress and strain information is provided in the “Trimming” process in the eZ-Setup for 
users to set up a trimming input deck under the circumstance. 
2D and 3D trimming of solid elements and laminates: 
Trimming curve preparation, file inclusion, etc. 
The  requirement  for  trimming  curves  definition  of  solids  in  case  of  3D  trimming  is 
different from that of shell trimming.  The trim curve should be created based on solid 
element  normal.    If  trim  curve  is  created  closer  to  the  top  surface,  the  variable  TDIR 
should be set to 1; if closer to the bottom surface, set to -1, see Figure 15-27. 
Normal directions of solid elements can be viewed using LS-PrePost starting in version 
4.2 with the menu option of EleTol → Normal → Entity Type: Solid → By Part, and set a 
large V-Size.  In addition, when defining a trim curve for the 3D trimming of both solids 
and laminates, the curve should be as close to either the top or bottom side of the part 
as  possible  to  enable  a  successful  trimming.    This  is  especially  true  if  wrinkles  are 
present in the panels to be trimmed.  LS-PrePost can be used to project the curves to the 
part, via menu option: GeoTol → Project → Closest proj → Project to Element.  Either top or 
bottom side of the part can be selected as “Element” by part.  The curves may need to be 
refined  with  more  points  before  projection,  using  menu  option:  Curves  →  Method: 
Respace → By number.  Sufficient number of points may be entered to capture the sheet 
metal surface contour. 
For  solid  element  trimming,  only  *INCLUDE_TRIM  (not  *INCLUDE)  is  supported  to 
include the dynain file from a previous process (for example, forming) simulation. 
2D trimming of solid elements 
As of Revision 92088, 2D (option NEW) trimming in any direction (defined by a vector) 
of solid elements is available.  An illustration of the 2D trim is shown in Figure 15-25.  A 
partial  keyword  example  is  provided  below,  where  trim  curves  trimcurves2d.iges  is 
being used to perform a solid element trimming along a vector defined along the global 
Z-axis. 
*KEYWORD 
*INCLUDE_TRIM 
incoming.dynain 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*PARAMETER_EXPRESSION 
...
*CONTROL_TERMINATION 
$   ENDTIM 
0.0 
*CONTROL_OUTPUT 
... 
*DATABASE_XXX 
... 
*PART 
 Solid Blank 
$#     pid     secid       mid 
  &blk1pid  &blk1sec  &blk1mid 
*SECTION_Solid 
&blk1sec,&elform 
*MAT_PIECEWISE_LINEAR_PLASTICITY 
... 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
$   Trim cards 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*CONTROL_FORMING_TRIMMING 
$     PSID 
   &blksid 
*DEFINE_TRIM_SEED_POINT_COORDINATES 
$ NSEED,X1,Y1,Z1,X2,Y2,Z2 
1,&seedx,&seedy,&seedz 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*DEFINE_CURVE_TRIM_NEW 
$#    tcid    tctype      tflg      tdir     tctol      toln    nseed1    nseed2 
         2         2         0         1   0.10000  1.000000         0         0 
$# filename 
trimcurves2d.iges 
*DEFINE_VECTOR 
$#     vid        xt        yt        zt        xh        yh        zh       cid 
         1     0.000     0.000     0.000     0.000     0.000  1.000000         0 
*INTERFACE_SPRINGBACK_LSDYNA 
$     PSID 
&blksid,&nshv 
*END 
Currently, 2D trimming of solids in some cases may be approximate.  The trimming will 
trim the top and bottom sides of the elements, not crossing over to the other sides.  This 
can be seen, for instance, trimming involving a radius. 
3D (normal) trimming of solid elements 
As of Revision 93467 3D trimming (option 3D) of solid elements is available.  From the 
previous  input,  in  case  of  3D  trimming,  the  option  NEW  is  changed  to  3D,  and  trim 
curves trimcurves3d.iges is used.  In the example below, the variable TDIR is set to “1” 
since the trim curve is on the positive side of the element normal (Figure 15-27).  Since 
3D  trimming  are  along  the  element  normal  directions,  *DEFINE_VECTOR  card  is  no 
longer needed. 
*DEFINE_CURVE_TRIM_3D 
$#    tcid    tctype      tflg      tdir     tctol      toln    nseed1    nseed2 
         2         2         0         1   0.10000  1.000000         0         0 
$# filename 
trimcurves3d.iges 
Again, the projection of trim curves onto either the top or bottom surface of the blank is 
important to ensure a smooth and successful trimming.
2D and 3D trimming of non-adaptive-meshed sandwiched parts (laminates) 
2D  and  3D  trimming  of  non-adaptive-meshed  laminates  are  available  starting  in 
Revision 92289.  Trimming of the laminates can have multiple layers of solid elements, 
sandwiched by a top and a bottom layer of shell elements.  Note that the nodes of shell 
elements  must  share  the  nodes  with  solid  elements  at  the  top  and  bottom  layers.    An 
illustration of the trim is shown in Figure 15-26.  The input deck is similar to those used 
for  trimming  of  solid  elements,  except  the  variable  ITYP  under  *CONTROL_FORM-
ING_TRIMMING should be set to “1” to activate the trimming of laminates in both 2D 
and 3D conditions: 
*CONTROL_FORMING_TRIMMING 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
$     PSID                ITYP 
   &blksid                   1 
Again, in the case of 3D trimming, the projection of trim curves onto either the top or 
bottom surface of the blank is important to ensure a smooth and successful trim. 
2D and 3D trimming of adaptive-meshed sandwiched parts (laminates) 
2D  and  3D  trimming  of  adaptive-meshed  laminates  are  available  starting  in  Revision 
108770.    Trimming  of  the  laminates  is  limited  to  one  core  layer  of  solid  elements, 
sandwiched  by  a  top  and  a  bottom  layer  of  shell  elements.    Shell  elements  share  the 
same nodes as the solid elements. 
the 
cut  by 
Note  elements  are  refined  automatically  along  the  trim  curves  until  no  slave  nodes 
would  be 
the  keyword 
curves. 
*CONTROL_ADAPTIVE_CURVE must not be used, since it is only applied to shell 
elements,  and  would  cause  error  termination  otherwise.    Furthermore,  unlike  the 
mesh  refinement  along  the  trim  curve  during  shell  element  trimming,  this  trimming 
requires no additional adaptivity-related keyword inputs.  An example of the trimming 
on the 2005 NUMISHEET Cross Member is shown in Figure 15-28. 
addition, 
trim 
In 
Again, in the case of 3D trimming, the projection of trim curves onto either the top or 
bottom surface of the blank is important to ensure a smooth and successful trim. 
Summary – trimming of solids and laminates 
In summary, the trimming input files between solids/laminates and shells are different 
in a few ways.  For solids, *SECTION_SOLID is needed in place of *SECTION_SHELL.  
For  laminates,  in  addition  to  setting  the  ITYP = 1  in  *CONTROL_FORMING_TRIM-
MING,  both  *SECTION_SHELL  and  *SECTION_SOLID  need  to  be  defined.    The 
position  of  a  trim  curve  for  3D  trimming  of  solids  needs  to  be  defined  according  to 
Figure 15-27.
Adaptive-meshed sandwiched parts (limit to a core of one layer of solid elements with 
outer layers of shell elements) can be 2D or 3D trimmed with adaptive mesh refinement 
along the trim curves. 
Non-adaptive-meshed  sandwiched  parts  (a  core  of  multiple  layers  of  solid  elements 
with outer layers of shell elements) can be 2D and 3D trimmed. 
In  all  trimming  of  solids  and  laminates,  only dynain  file  is  written  out  (no d3plot  files 
will be output), and finally, *INCLUDE_TRIM is to be used. 
In the case of 3D trimming, the projection of trim curves onto either the top or bottom 
surface of the blank is important to ensure a smooth and successful trim. 
2D trimming of thick shell elements (TSHELL): 
2D  trimming  of  TSHELL  is  supported  starting  from  Revision  107957.    Note  by 
definition,  TSHELL  has  only  one  layer  of  solid  elements,  and  is  defined  by  keyword 
*SECTION_TSHELL.    Note  also  *INCLUDE_TRIM  (not  *INCLUDE)  must  be  used  to 
include the dynain file to be trimmed. 
Input deck for 2D trimming of TSHELL is similar to what is used for trimming of solid 
elements. 
2D and 3D trimming of double-attached solids and laminates: 
These  features  are  available  starting  in  Revision  110140.    Both  seed  point  coordinates 
can  be  specified  in  *DEFINE_TRIM_SEED_POINT_COORDINATES  to  define  a  seed 
coordinate for each part, as shown below: 
*DEFINE_TRIM_SEED_POINT_COORDINATES 
$    NSEED        X1        Y1        Z1        X2        Y2        Z2 
         2  -184.565    84.755    78.392  -1038.41   119.154    78.375 
In  Figure  15-29,  a  2D double-trimming  example  on a  sandwiched  part  is  shown  using 
the 2005 NUMISHEET cross member.  Two trim curves, two seed nodes are defined for 
each  to  be  trimmed  portion.    The  coordinates  for  seed  node  #1  is  (-184.565,  84.755, 
78.392)  and  is  (-1038.41,  119.154,  78.375)  for  seed  node  #2.    Trimmed  results  are 
satisfactory. 
Revision information: 
Revision information are as follows:
1.  Revision 54608 and 52312: negative seed node option is available for the options 
3D and NEW, respectively. 
2.  Revision  65630:  Use  of  TCTOL  as  a  distance  for  mesh  refinement  (when  used 
together with *CONTROL_ADAPTIVE_CURVE) is available. 
3.  Revision 68643: trimming is enabled for those trim lines going beyond the part 
boundary. 
4.  Revision 92088: 2D (option NEW) trimming of solid elements. 
5.  Revision 92289: 2D and 3-D (option 3D) trimming of laminates. 
6.  Revision 93467: 3D trimming of solid elements. 
7.  Revision 101964: TDIR definition activated for 3D trimming of top and bottom 
surfaces of solid elements and laminates. 
8.  Revision 107957: 2D trimming of TSHELL. 
9.  Revision 109047: 2D and 3D trimming of adaptive-meshed sandwiched part. 
10.  Revision  110140:  2D  and  3D  trimming  of  solids  and  laminates  of  double-
attached parts. 
11.  Latter Revisions may incorporate more improvements and are suggested to be 
used for trimming.
Part to be trimmed
Trim curve 
(local system)
Trim curve 
(projected)
Figure 15-18.  Trimming Orientation Vector.  The tail (T) and head (H) points 
define  a  local  coordinate  system  (x,y,z).    The  global  coordinate  system  is
named (X,Y,Z).  The local x-direction is constructed in the Xz plane.  If X and z
nearly  coincide  (|X  •  z| > 0.95),  then  the  local  x-direction  is  instead 
constructed  in  the  Yz  plane.    Trim  curve  data  is  input  in  the  x-y  plane,  and 
projected in the z-direction onto the deformed mesh to obtain the trim line. 
Tol = 0.25 (default)
Tol = 0.01
Figure 15-19.  Trimming Tolerance.  The tolerance limits the size of the small
elements  generated  during  trimming.    The  default  tolerance  (left)  produces
large elements.  Using a tolerance of 0.01 (right) allows smaller elements, and
more detail in the trim line.
Seed nodes
Trim line
18764
43356
Punch opening line
Figure 15-20.  Trimming of a double-attached part (NUMISHEET2002 Fender 
Outer). 
Blank edge line
Punch opening line
Figure 15-21.  The fender outer (draw complete) in wireframe mode.
Figure 15-22.  The fender outer - thickness/thinning plot on the drawn panel. 
Figure  15-23.    The  fender  outer  trim  complete  using  the  NSEED1/NSEED2
feature.
Blank edge outline
Trim line loops outside 
of the part periphery
Punch opening line
Figure 15-24.  Revision 68643 deals with trim curves going beyond part 
boundary.
Trim curves 
in red 
Three layers of solid 
elements through the 
thickness
Trim vectors
  Figure 15-25.  2-D trimming of solids using *DEFINE_CURVE_TRIM_NEW
Top layer of shell elements
Five-layers  of  3-D 
solid elements
Trim curves 
(piecewise)
Bottom layer of shell elements
Figure  15-26.    3-D  trimming  of  laminates  (a  core  of  multiple-layers  of  solid
elements  with 
shell  elements)  using
*DEFINE_CURVE_TRIM_3D.    Note  that  shell  elements  must  share  the  same
nodes with the solid elements at the top and bottom layer. 
top  and  bottom 
layers  of 
Positive side of solid element normals; 
check solid normals using LS-PrePost4.2
Trim curve
All solid element normals must be consistent.  If trim curve is close to the 
positive normal side, set TDIR=1; otherwise set TDIR=-1.  Respacing the 
curve with more points, project the respaced curve to the top or bottom 
solid surface may help the trimming. 
  Figure 15-27.  Define trim curve for 3D trimming of solid and laminates.
Inner trim curve
Outer trim curve
Elements (both shells and solids) are 
automatically refined along the trim curves
Mesh prior to trim
Trimmed mesh
Trim curves
Drawn Panel
2005 NUMISHEET Cross Member - 
Drawn Panel and Trim Curves
Figure 15-28.  Trimming of an adaptive mesh on a sandwiched part.  Meshes
are  automatically  refined  along  the  trim  curves.    Note  that  only  one  layer  of
solid element as a core is allowed for adaptive-meshed sandwich parts.  Also
top and bottom layer of shells must share the same nodes as the solid elements.
The keyword *CONTROL_ADAPTIVE_CURVE must not be used.
Trim curve #1
Drawn Panel
Trimmed piece #1
*DEFINE 
Trim direction: 
global Z
Trim curve #2
Seed node #2
Trimmed piece #2
Trim curves, seed nodes and 
direction defintion
Trimmed results
Figure 15-29.  An example of 2D trimming of sandwiched part (laminates) 
from  
2005 NUMISHEET benchmark - cross member.
*DEFINE_DEATH_TIMES_OPTION 
Available options include: 
NODES 
SET 
RIGID 
Purpose:  To dynamically define the death times for *BOUNDARY_PRESCRIBED_MO-
TION  based  on  the  locations  of  nodes  and  rigid  bodies.    Once  a  node  or  rigid  body 
moves past a plane or a geometric entity, the death time is set to the current time.  The 
input in this section continues until the next ‘*’ card is detected. 
5 
6 
7 
8 
  Card 1 
1 
Variable 
GEO 
Type 
I 
Default 
  Card 2 
1 
2 
N1 
I 
0 
2 
3 
N2 
I 
0 
3 
4 
N3 
I 
0 
4 
5 
6 
Variable 
X_T 
Y_T 
Z_T 
X_H 
Y_H 
Z_H 
Type 
F 
F 
F 
F 
F 
F 
Default 
7 
R 
F 
8 
FLAG 
1 
ID Cards.  Set the list of nodes and rigid bodies affected by this keyword.  This input 
terminates at the next keyword (“*”) card.  
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSID1 
NSID2 
NSID3 
NSID4 
NSID5 
NSID6 
NSID7 
NSID8 
Type 
I 
I 
I 
I 
I 
I 
I
GEO = 1
GEO = 3
GEO = 2
O = origin
= X_T, Y_T, Z_T or
coordinates of N1
V = X_H - X_T, Y_H - Y_T,
Z_H - Z_T or coordinates
of N3 - coordinates of N2
Figure 15-30.  Geometry types. 
  VARIABLE   
DESCRIPTION
GEO 
Geometric entity type. = 1 plane, = 2 infinite cylinder, = 3 sphere 
N1 
N2 
N3 
X_T 
Y_T 
Z_T 
X_H 
Y_H 
Z_H 
R 
Node defining the origin of the geometric entity (optional). 
Node defining the tail of the orientation vector (optional). 
Node defining the head of the orientation vector (optional). 
X  coordinate  of  the  origin  of  the  geometric  entity  and  the  tail  of
the orientation vector. 
Y  coordinate  of  the  origin  of  the  geometric  entity  and  the  tail  of 
the orientation vector. 
Z  coordinate  of  the  origin  of  the  geometric  entity  and  the  tail  of
the orientation vector. 
X coordinate of the head of the orientation vector. 
Y coordinate of the head of the orientation vector. 
Z coordinate of the head of the orientation vector. 
Radius of cylinder or sphere.
FLAG 
*DEFINE_DEATH_TIMES 
DESCRIPTION
+1  for  killing  motion  when  the  node  is  outside  of  the  geometric
entity  or  on  the  positive  side  of  the  plane  as  defined  by  the
normal direction, or -1 for the inside. 
NSIDi 
i-th node, node set, or rigid body 
Remarks: 
1.  Either N1 or X_T, Y_T, and Z_T should be specified, but not both. 
2.  Either N2 and N3 or X_H, Y_H, and Z_H should be specified, but not both.  If 
N2 and N3.  Specifying N2 and N3 is equivalent of setting the head of the vec-
tor equal to the tail of the vector (X_T, Y_T, and Z_T) plus the vector from N2 to 
N3.
*DEFINE 
Purpose:  To define an interested region for Discrete Elements (DE) for high efficiency 
collision  pair  searching.    Any  DE  leaving  this  domain  will  not  be  considered  in  the 
future DE searching and also disabled in the contact algorithm. 
6 
7 
8 
  Card 1 
Variable 
1 
ID 
2 
3 
TYPE 
Xm 
Type 
I 
Default 
none 
I 
0 
F 
0. 
4 
Ym 
F 
0. 
5 
Zm 
F 
0. 
  VARIABLE   
DESCRIPTION
ID 
TYPE 
Set ID/Box ID 
EQ.0: Part set ID 
EQ.1: Box ID 
Xm, Ym, Zm 
Factor  for  region's  margin  on  each  direction  based  on  region
length. 
The  static  coordinates limits  are  determined either  by  part  set  or
box  option.    To  extended  those  limits  to  provide  a  buffer  zone,
these  factors  can  be  used.    The  margin  in  each  direction  is
calculated in the following way: 
Let 𝑋max and 𝑋min be the limits in the x direction.  Then, 
Then the margin is computed from the input as, 
Δ𝑋 = 𝑋max − 𝑋min 
𝑋margin = Xm × Δ𝑋 
Then the corresponding limits for the active region are, 
𝑋max
′ = 𝑋max   +   𝑋margin 
′ = 𝑋min − 𝑋margin
𝑋min
*DEFINE_DE_BOND 
Purpose:  To define a bond model for discrete element sphere (DES). 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
STYPE 
BDFORM 
Type 
I 
Default 
none 
I 
0 
I 
1 
  VARIABLE   
DESCRIPTION
SID 
DES nodes 
STYPE 
EQ.0: DES node set 
EQ.1: DES node 
EQ.2:  DES part set 
EQ.3: DES part 
BDFORM 
Bond formulation: 
EQ.1: Linear bond formulation. 
Card 2 for BDFORM = 1. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PBN 
PBS 
PBN_S 
PBS_S 
SFA 
ALPHA 
MAXGA
P 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
1.0 
0.0 
1.E-4 
  VARIABLE   
DESCRIPTION
PBN 
Parallel-bond modulus [Pa].  See Remark 1
VARIABLE   
DESCRIPTION
PBS 
PBN_S 
PBS_S 
Parallel-bond stiffness ratio.  shear stiffness/normal stiffness.  See
Remark 2 
Parallel-bond  maximum  normal  stress.    A  zero  value  defines  an
infinite maximum normal stress. 
Parallel-bond  maximum  shear  stress.    A  zero  value  defines  an
infinite maximum shear stress. 
SFA 
Bond radius multiplier 
ALPHA 
Numerical damping 
MAXGAP 
Maximum gap between two bonded spheres 
GT.0.0: defines  the  ratio  of  the  smaller  radius  of  two  bonded
  MAXGAP  ×
spheres  as  the  maximum  gap,  i.e. 
min(r1,r2) 
LT.0.0:  absolute value is used as the maximum gap. 
Remarks: 
1.The normal force is calculated as 
× A × ∆𝑢𝑛 
∆𝑓n =
𝑃𝐵𝑁
(𝑟0 + 𝑟1)
where 
2  
𝐴 = 𝜋𝑟𝑒𝑓𝑓
𝑟𝑒𝑓𝑓 = 𝑚𝑖𝑛(𝑟0, 𝑟1) × 𝑆𝐹𝐴 
2.The shear force is calculated as 
∆𝑓s = PBS ×
𝑃𝐵𝑁
(𝑟0 + 𝑟1)
× A × ∆𝑢𝑠
*DEFINE_DE_BY_PART 
Purpose:    To  define  control  parameters  for  discrete  element  sphere  by  part  ID.    This 
card overrides the values set in *CONTROL_DISCRETE_ELEMENT. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
NDAMP 
TDAMP 
FRICS 
FRICR 
NORMK 
SHEARK 
Type 
I 
Default 
none 
  Card 2 
1 
F 
0 
2 
F 
0 
3 
F 
0 
4 
F 
0 
5 
F 
F 
0.01 
2/7 
6 
7 
8 
Variable 
GAMMA 
VOL 
ANG 
Type 
Default 
F 
0 
F 
0 
F 
0 
Card 3 is optional 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LNORM 
LSHEAR 
FRICD 
DC 
Type 
Default 
I 
0 
I 
0 
  VARIABLE   
F 
FRICS 
F 
0 
DESCRIPTION
PID 
Part ID of DES nodes 
NDAMP 
Normal damping coefficient 
TDAMP 
Tangential damping coefficient
DESCRIPTION
  VARIABLE   
FRICS 
Static coefficient of friction.  The  frictional coefficient is assumed
to  be  dependent  on  the  relative  velocity  𝑣𝑟𝑒𝑙of  the  two  DEM  in 
contact 𝜇𝑐 = 𝐹𝑅𝐼𝐶𝐷 + (𝐹𝑅𝐼𝐶𝑆 − 𝐹𝑅𝐼𝐶𝐷)𝑒−𝐷𝐶∙∣𝑣𝑟𝑒𝑙∣. 
EQ.0: 3 DOF 
NE.0:  6 DOF (consider rotational DOF) 
FRICR 
Rolling friction coefficient 
NORMK 
Optional: scale factor of normal spring constant (Default = 0.01) 
SHEARK 
Optional: ratio between ShearK/NormK (Default = 2/7) 
GAMMA 
Liquid surface tension 
VOL 
ANG 
LNORM 
LSHEAR 
FRICD 
Volume fraction 
Contact angle 
Load curve ID of a curve that defines function for normal stiffness
with respect to norm penetration ratio 
Load curve ID of a curve that defines function for shear stiffness
with respect to norm penetration ratio 
Dynamic coefficient of friction.  By default, FRICD = FRICS.  The 
frictional  coefficient  is  assumed  to  be  dependent  on  the  relative
velocity  𝑣𝑟𝑒𝑙of  the  two  DEM  in  contact  𝜇𝑐 = 𝐹𝑅𝐼𝐶𝐷 + (𝐹𝑅𝐼𝐶𝑆 −
𝐹𝑅𝐼𝐶𝐷)𝑒−𝐷𝐶∙∣𝑣𝑟𝑒𝑙∣. 
DC 
Exponential  decay  coefficient. 
  The  frictional  coefficient  is
assumed  to  be  dependent  on  the  relative  velocity  𝑣𝑟𝑒𝑙of  the  two 
DEM in contact 𝜇𝑐 = 𝐹𝑅𝐼𝐶𝐷 + (𝐹𝑅𝐼𝐶𝑆 − 𝐹𝑅𝐼𝐶𝐷)𝑒−𝐷𝐶∙∣𝑣𝑟𝑒𝑙∣. 
See also *CONTROL_DISCRETE_ELEMENT.
*DEFINE_DE_HBOND 
Purpose:  To define a heterogeneous bond model for discrete element sphere (DES). 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
STYPE 
HBDFM 
IDIM 
Type 
I 
Default 
none 
I 
0 
I 
1 
I 
3 
  VARIABLE   
DESCRIPTION
SID 
DES nodes 
STYPE 
EQ.0: DES node set 
EQ.1: DES node 
EQ.2:  DES part set 
EQ.3: DES part 
HBDFM 
Bond formulation: 
EQ.1: (Reserved) 
EQ.2: Nonlinear  heterogeneous  bond  formulation  for  fracture
analysis based on the general material models defined in
the material cards.  DES elements with different material
models can be defined within one bond. 
IDIM 
Space dimension for DES bonds: 
EQ.2: for 2D plane strain problems 
EQ.3: for 3D problems.
*DEFINE 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PBK_SF 
PBS_SF 
FRGK 
FRGS 
BONDR 
ALPHA 
DMG 
FRMDL 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
1.0 
1.0 
none 
none 
none 
0.0 
1.0 
I 
1 
  VARIABLE   
DESCRIPTION
PBK_SF 
Scale factor for volumetric stiffness of the bond. 
PBS_SF 
Scale factor for shear stiffness of the bond. 
FRGK 
Critical  fracture  energy  release  rate  for  volumetric  deformation
due to the hydrostatic pressure. 
Special Cases: 
EQ.0: A  zero  value  specifies  an  infinite  energy  release  rate  for 
unbreakable bonds. 
LT.0:  A  negative  value  defines  the  energy  release  rate  under
volumetric  compression  (i.e.    positive  pressure)  and
FRGS defined below is used under volumetric expansion
(i.e.  negative pressure). 
FRGS 
Critical fracture energy release rate for shear deformation. 
Special Cases: 
EQ.0: 
A  zero  value  specifies  an  infinite  energy  release
rate for unbreakable bonds. 
FRGK.LT.0: See description for FRGK 
BONDR 
Influence radius of the DES nodes.  
ALPHA 
Numerical damping
*DEFINE_DE_HBOND 
DESCRIPTION
DMG 
Continuous parameter for damage model. 
EQ.1.0:  The  bond  breaks  if  the  fracture  energy  in  the  bond
reaches the critical value.  Microdamage is not calcu-
lated. 
∈ (0.5,1): Microdamage  effects  being  once  the  fracture  energy
reaches DMG × FMG[K,S].  Upon the onset of micro-
damage,  the  computed  damage  ratio  will  increase
(monotonically)  as  the  fracture  energy  grows.    Bond
weakening  from  microdamage  is  modeled  by  reduc-
ing the bond stiffness in proportion to the damage ra-
tio. 
FRMDL 
Fracture model: 
EQ.1:  Fracture  energy  of  shear  deformation  is  calculated
based on deviatoric stresses. 
EQ.2:  Fracture  energy  of  shear  deformation  is  calculated
based  on  deviatoric  stresses,  excluding  the  axial  compo-
nent (along the bond). 
EQ.3,4:  Same  as  1&2,  respectively,  but  FRGK  and  FRGS  are 
read as the total failure energy density and will be con-
verted to the corresponding critical fracture energy re-
lease rate.  The total failure energy density is calculated
as  the  total  area  under  uniaxial  tension  stress-strain 
curve. 
EQ.5,6:  Same as 3&4, respectively, as FRGK and FRGS are read
as  the  total  failure  energy  density  but  will  not  be  con-
verted.  Instead, the failure energy within the bond will
be calculated. 
Models  1&2  are  more  suitable  for  brittle  materials,  and  Models 
5&6 are easier for ductile materials.  Models 3&4 can be used for
moderately ductile fracture accordingly. 
This  is  the  default  fracture  model  and  applied  to  all  DES  parts,
even  if  they  have  different  material  models.    More  fracture
models  can  be  defined  for  different  materials  by  specifying  an 
interface ID (ITFID) in the optional card.
Pre-crack Card.  This card is optional. 
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PRECRK 
CKTYPE 
ITFID 
Type 
I 
Default 
none 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
PRECRK 
Shell set, define 3D surfaces of the pre-crack 
CKTYPE 
ITFID 
EQ.0: Part set 
EQ.1: Part 
ID  of  the  interface  *INTERFACE_DE_HBOND,  which  defines
different failure models for the heterogeneous bonds within each
part and between two parts respectively.
*DEFINE_DE_INJECTION_{OPTION} 
Available options include: 
<BLANK> 
ELLIPSE 
Purpose:  This keyword injects discrete element spheres (DES) from specified a region 
at a flow rate given by a user defined curve.  When the option is blank the region from 
which the DES emanate is assumed rectangular.  The elliptical option indicates that the 
region is to be elliptical. 
  Card 1 
1 
Variable 
PID 
2 
SID 
Type 
I 
I 
3 
XC 
F 
4 
YC 
F 
5 
ZC 
F 
6 
XL 
F 
7 
YL 
F 
Default 
none 
none 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 2 
1 
2 
3 
4 
Variable 
RMASS 
RMIN 
RMAX_S 
VX 
Type 
F 
F 
F 
F 
5 
VY 
F 
6 
VZ 
F 
7 
TBEG 
TEND 
F 
F 
Default 
none 
none 
RMIN 
0.0 
0.0 
0.0 
0.0 
1020 
Optional card. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IFUNC 
Type 
Default 
I 
0 
15-140 (DEFINE) 
LS-DYNA R10.0 
8 
CID
VARIABLE   
DESCRIPTION
PID 
SID 
Part ID of new generated DES nodes 
  Nodes  and  DES  properties  are  generated
Node  set  ID. 
automatically  during  input  phase  based  on  the  user  input  and
assigned to this SID. 
XC, YC, ZC 
𝑥, 𝑦, 𝑧 coordinate of the center of injection plane 
XL 
YL 
CID 
For rectangular planes XL specifies the planar length along the 𝑥-
axis  in  the  coordinate  system  specified  by  CID.    For  elliptical
planes XL specifies the length of the major axis. 
For rectangular planes YL specifies the planar length along the 𝑦-
axis  in  the  coordinate  system  specified  by  CID.    For  elliptical
planes YL specifies the length of the minor axis. 
Optional  local  coordinate  system  ID,  see  *DEFINE_COORDI-
NATE_SYSTEM 
RMASS 
Mass flow rate 
LT.0:  Curve ID 
RMIN 
Minimum DES radius 
RMAX 
Maximum DES radius 
VX, VY, VZ 
Vector  components  defining  the  initial  velocity  of  injected  DES
specified relative the coordinate system defined by CID. 
Birth time 
Death time 
EQ.0:  Uniform distribution(Default) 
EQ.1:  Gaussian distribution (Remark 1) 
TBEG 
TEND 
IFUNC 
Remarks: 
The distribution of particle radius follows Gaussian distribution  
𝑓 (𝑟∣𝑟0, 𝜎) =
−
(𝑟−𝑟0)2
2𝜎 2
𝜎√2𝜋
Where the mean radius is given by
and the standard deviation is 
𝑟0 =
𝜎 =
(𝑟max + 𝑟min), 
(𝑟max − 𝑟min)
*DEFINE 
Purpose:    To  measure  DES  mass  flow  rate  across  a  defined  plane.    See  also  the 
accompanying  keyword  *DATABASE_DEMASSFLOW  which  controls  the  output 
frequency. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SLAVE  MASTER 
STYPE 
MTYPE 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
  VARIABLE   
SLAVE 
DESCRIPTION
Node set ID, node ID, part set ID or part ID defining DES on slave
side.  STYPE below indicates the ID type specified by SLAVE. 
MASTER 
Part  set  ID  or  part  ID  defining  master  surface.    MTYPE  below
indicates the ID type specified by MASTER. 
STYPE 
Slave type. 
EQ.0: Slave node set 
EQ.1: Slave node 
EQ.2: Slave part set 
EQ.3: Slave part 
MTYPE 
Master type. 
EQ.0: Part set 
EQ.1: Part
*DEFINE_DE_TO_BEAM_COUPLING 
Purpose:    To  define  coupling  interface  between  discrete  element  sphere  (DES)  and 
beam. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SLAVE  MASTER 
STYPE 
MTYPE 
Type 
Default 
I 
0 
  Card 2 
1 
I 
0 
2 
I 
0 
3 
I 
0 
4 
Variable 
FricS 
FricD 
DAMP 
BSORT 
Type 
Default 
F 
0 
F 
0 
F 
0 
I 
100 
5 
6 
7 
8 
  VARIABLE   
DESCRIPTION
SLAVE 
DES nodes 
MASTER 
Shell set 
STYPE 
MTYPE 
FricS 
FricD 
EQ.0: Slave node set 
EQ.1: Slave node 
EQ.2: Slave part set 
EQ.3: Slave part 
EQ.0: Part set 
EQ.1: Part 
Friction coefficient 
Rolling friction coefficient
VARIABLE   
DESCRIPTION
DAMP 
Damping coefficient 
BSORT 
Number of cycle between bucket sortings.  (Default = 100)
*DEFINE_DE_TO_SURFACE_COUPLING 
Purpose:    To  define  a  non-tied  coupling  interface  between  discrete  element  spheres 
(DES) and a surface defined by shell part(s) or solid part(s).  This coupling is currently 
not implemented for tshell part(s). 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SLAVE  MASTER 
STYPE 
MTYPE 
Type 
Default 
I 
0 
  Card 2 
1 
I 
0 
2 
I 
0 
3 
I 
0 
4 
5 
6 
7 
8 
Variable 
FricS 
FricD 
DAMP 
BSORT 
LCVx 
LCVy 
LCVz 
WEARC 
Type 
Default 
F 
0 
F 
0 
F 
0 
I 
100 
I 
0 
I 
0 
I 
0 
User Defined Wear Parameter Cards.  Additional Card for WEARC.LT.0.  
  Card 3 
1 
Variable 
W1 
2 
W2 
3 
W3 
4 
W4 
5 
W5 
6 
W6 
7 
W7 
F 
0. 
8 
W8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none
Card 4 is optional.  
  Card 4 
1 
2 
3 
4 
5 
6 
7 
Variable 
SFP 
SFT 
CID_RCF 
BT 
Type 
F 
F 
Default 
1.0 
1.0 
I 
0 
F 
0 
8 
DT 
F 
1.E20 
  VARIABLE   
SLAVE 
MASTER 
STYPE 
MTYPE 
FricS 
FricD 
DAMP 
DESCRIPTION
Node  set  ID,  node  ID,  part  set  ID  or  part  ID  defining  DES    on
slave  side.    STYPE  below  indicates  the  ID  type  specified  by
SLAVE. 
Part  set  ID  or  part  ID  defining  master  surface.    MTYPE  below
indicates the ID type specified by MASTER. 
EQ.0: Slave node set 
EQ.1: Slave node 
EQ.2: Slave part set 
EQ.3: Slave part 
EQ.0: Part set 
EQ.1: Part 
Friction coefficient 
Rolling friction coefficient 
Damping  coefficient  (unitless).    If  a  discrete  element  sphere
impacts  a  rigid  surface  with  a  velocity  𝑣impact,  the  rebound 
velocity is 
𝑣rebound = (1 − DAMP)𝑣impact
BSORT 
*DEFINE_DE_TO_SURFACE_COUPLING 
DESCRIPTION
Number  of  cycle  between  bucket  sortings;  Default  value  is  100. 
For  blast  simulation  with  very  high  DEM  particles  velocity,  it  is
suggested to set BSORT = 20 or smaller. 
LT.0: ABS(BSORT)  is  the  minimum  number  of  cycle  between
bucket sort.  This value can be increased during runtime
by  tracking  the  velocity  of  potential  coupling  pair.    This
feature only works with MPP currently. 
LVCx 
LVCy 
LVCz 
Load curve defines surface velocity in 𝑥 direction 
Load curve defines surface velocity in 𝑦 direction 
Load curve defines surface velocity in 𝑧 direction 
WEARC 
WEARC is the wear coefficient.  
GT.0: 
EQ.-1: 
Archard’s Wear Law, See Remark 1. 
Finnie Wear Law, additional card is required 
EQ.-100: User defined wear model, additional card is required
W1-W8 
WEARC = -1, W1 is yield stress of target material 
WEARC = -100, user defined wear parameters 
SFP 
SFT 
Scale  factor  on  contact  stiffness.    By  default,  SFP = 1.0.    The 
as
contact 
calculated 
stiffness 
is 
𝐾𝑛 = 𝑆𝐹𝑃 ∙ {
𝐾 ∙ 𝑟 ∙ 𝑁𝑜𝑟𝑚𝐾  𝑖𝑓  𝑁𝑜𝑟𝑚𝐾 > 0
|𝑁𝑜𝑟𝑚𝐾|  𝑖𝑓  𝑁𝑜𝑟𝑚𝐾 < 0
  where  K 
is  bulk 
modulus, r is discrete element radius, NormK is scale factor of the 
spring constant defined in *CONTROL_DISCRETE_ELEMENT. 
Scale  factor  for  surface  thickness  (scales  true  thickness).    This
option applies only to contact with shell elements.  True thickness
is the element thickness of the shell elements. 
CID_RCF 
Coordinate  system  ID to output demrcf  force resultants  in  a  local 
system. 
BT 
DT 
Birth time. 
Death time.
Remarks: 
1.  Archard’s  Wear  Law.    If  WEARC > 0  then  wear  on  the  shell  surface  is 
calculated using Archard’s wear law 
ℎ̇ =
WEARC × 𝑓𝑛 × 𝑣𝑡
where, 
ℎ = wear depth 
𝑓𝑛 = normal contact force from DE 
𝑣𝑡 = tangential sliding velocity of the DE on shell 
𝐴 = area of contact segment 
The wear depth is output to the interface force file. 
2.  Finnie’s Wear Law.  If WEARC=-1 then wear on the shell surface is calculated 
using Finnie’s wear law.  The model of Finnie relates the rate of wear to the rate 
of kinetic energy of particle impact on a surface as: 
Q =
⎧ 𝑚𝑣2
{{{
8𝑝
⎨
𝑚𝑣2
{{{
24𝑝
⎩
(sin 2𝛼 − 3 sin2 𝛼)  𝑖𝑓   tan 𝛼 <
cos2 𝛼                         𝑖𝑓   tan 𝛼 >
where,  Q  is  the  volume  of  the  material  removed  from  surface,  m  is  particle 
mass, α is impact angle and p is the yield stress of the target material, p is read 
from additional user defined wear parameter card as p = w1..  The wear depth 
is output to the interface force file.  
3. 
*DATABASE_BINARY_DEMFOR  controls  the  output  interval  of  the  coupling 
forces to the DEM interface force file. This interface force file is activated by the 
command line option “dem=”, for example, 
lsdyna i=inputfilename.k … dem=interfaceforce_filename 
The DEM interface force file can be read into LS-PrePost for plotting of coupling 
pressure and forces on the master segments. 
4. 
*DATABASE_RCFORC controls the output interval of the coupling forces to the 
ASCII  demrcf  file.    This  output  file  is  analogous  to  the  rcforc  file  for 
*CONTACT.
*DEFINE_DE_TO_SURFACE_TIED 
Purpose:    To  define  a  tied-with-failure  coupling  interface  between  discrete  element 
spheres  (DES)  and  a  surface  defined  by  shell  part(s)  or  solid  part(s).    This  coupling  is 
currently not implemented for tshell part(s). 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SLAVE  MASTER 
STYPE 
MTYPE 
Type 
Default 
I 
0 
  Card 2 
1 
I 
0 
2 
I 
0 
3 
I 
0 
4 
5 
6 
7 
8 
Variable 
NFLF 
SFLF 
NEN 
MES 
LCID 
NSORT 
Type 
F 
F 
F 
Default  Required  Required 
2. 
F 
2. 
I 
0 
I 
100 
  VARIABLE   
SLAVE 
MASTER 
STYPE 
DESCRIPTION
Node  set  ID,  node  ID,  part  set  ID  or  part  ID  defining  DES    on
slave  side.    STYPE  below  indicates  the  ID  type  specified  by
SLAVE. 
Part  set  ID  or  part  ID  defining  master  surface.    MTYPE  below
indicates the ID type specified by MASTER. 
EQ.0: Slave node set 
EQ.1: Slave node 
EQ.2: Slave part set 
EQ.3: Slave part 
MTYPE 
EQ.0: Part set 
EQ.1: Part
VARIABLE   
DESCRIPTION
NFLF 
SFLF 
NEN 
MES 
Normal  failure  force.    Only  tensile  failure,  i.e.,  tensile  normal
forces, will be considered in the failure criterion 
Shear failure force 
Exponent for normal force 
Exponent for shear force.  Failure criterion: 
(
∣𝑓𝑛∣
NFLF
NEN
)
+ (
∣𝑓𝑠∣
SFLF
MES
)
≥ 1. 
Failure is assumed if the left side is larger than 1.  𝑓𝑛 and 𝑓𝑠 are the 
normal and shear interface force. 
LCID 
Load curve ID define the time dependency of failure criterion 
NSORT 
Number of cycle between bucket sort 
Remarks: 
Both  NFLF  and  SFLF  must  be  defined.    If  failure  in  only  tension  or  shear  is  required 
then set the other failure force to a large value (1010).
*DEFINE_ELEMENT_DEATH_OPTION 
Available options include: 
SOLID 
SOLID_SET 
BEAM 
BEAM_SET 
SHELL 
SHELL_SET 
THICK_SHELL 
THICK_SHELL_SET 
Purpose:  To define a discrete time or box to delete an element or element set during the 
simulation.  This keyword is only for deformable elements, not rigid body elements. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EID/SID 
TIME 
BOXID 
INOUT 
IDGRP 
CID 
Type 
I 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
EID/SID 
Element ID or element set ID. 
TIME 
BOXID 
Deletion  time  for  elimination  of  the  element  or  element  set.    If
BOXID is nonzero, a TIME value of zero is reset to 1.0E+16. 
Element  inside  or  outside  of  defined  box  are  deleted  depending
on the value of INOUT. 
INOUT 
Location of deleted element: 
EQ.0: Elements inside box are deleted 
EQ.1: Element outside of box are deleted
VARIABLE   
IDGRP 
DESCRIPTION
Group  ID.    All  elements  sharing  the  same  positive  value  of
IDGRP are considered to be in the same group.  All elements in a
group  will  be  simultaneously  deleted  one  cycle  after  any  single
element in the group fails.   
There  is  no  requirement  that  each  *DEFINE_ELEMENT_DEATH 
command  have  a  unique  IDGRP.    In  other  words,  elements  in  a
single 
multiple
*DEFINE_ELEMENT_DEATH commands. 
group 
come 
from 
can 
Elements  in  which  IDGRP = 0  are  not  assigned  to  a  group  and 
thus  deletion  of  one  element  does  not  enforce  deletion  of  the 
other elements.   
CID 
Coordinate  ID  for  transforming  box  BOXID.    If  CID  is  not
specified,  the  box  is  in  the  global  coordinate  system.    The  box
rotates  and  translates  with  the  coordinate  system  only  if  the
coordinate system is flagged for an update every time step.
*DEFINE_ELEMENT_GENERALIZED_SHELL 
Purpose:  Define a general 3D shell formulation to be used in combination with *ELE-
MENT_GENERALIZED_SHELL.    The  objective  of  this  feature  is  to  allow  the  rapid 
prototyping  of  new  shell  element  formulations  by  adding  them  through  the  keyword 
input file. 
All necessary information, like the values of the shape functions and their derivatives at 
various locations (at the integration points and at the nodal points) have to be defined 
via  this  keyword.    An  example  for  a  9-noded  generalized  shell  element  with  4 
integration points in the plane is given in Figure 15-31 to illustrate the procedure.  The 
element formulation ID (called ELFORM) used in this keyword needs to be greater or 
equal than 1000 and  will be referenced through *SECTION_SHELL .  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ELFORM 
NIPP 
NMNP 
IMASS 
FORM 
Type 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
Weights and Shape Function Values/Derivatives at Gauss Points: 
These cards are read according to the following pseudo code: 
for i  = 1 to NIPP { 
read cardA1(i) 
for k = 1 to NMNP { 
read cardA2(i,k) 
} 
} // comment: Read in NIPP × (1 + NMNP) cards 
Weight Cards.  Provide weight for integration point i. 
 (Card A1)i 
Variable 
Type 
1 
2 
3 
4 
5 
6 
7 
8 
WI
Integration Point Shape Function Value/Derivatives Cards.  Provide the value of the 
kth shape function and its derivative at the ith integration point. 
(Card A2)ik 
Variable 
Type 
1 
2 
3 
4 
5 
6 
7 
8 
NKI 
F 
DNKIDR 
DNKIDS 
F 
F 
For FORM = 0 or FORM = 1, Shape Function Derivatives at Nodes: 
These cards are read according to the following pseudo code: 
for l  = 1 to NMNP { 
for k = 1 to NMNP { 
read cardB(l,k) 
} 
} // comment: Read in NMNP × NMNP cards 
Nodal  Shape  Function  Derivative  Cards.    The  value  of  the  kth  shape  function’s 
derivative at the lth nodal point. 
  (Card B)lk 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DNKLDR 
DNKLDS 
Type 
F 
F 
For FORM = 2 or FORM = 3, Shape Function 2nd derivative at Gauss Points: 
NOTE:  For FORM = 2 and FORM = 3 it is assumed that the 
shape functions are at least C1 continuous (having a 
continuous derivative). 
The cards for this method are read according to the following pseudo code:
for i  = 1 to NIPP { 
for k = 1 to NMNP { 
read cardB(l,k) 
} 
} // comment: Read in NGP × NMNP cards 
Nodal  Shape  Function  Second  Derivative  Cards.    The  value  of  the  kth  shape 
function’s second derivative at the ith integration point. 
(Card B)ik 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
D2NKIDR2 
D2NKIDRDS 
D2NKIDS2 
Type 
F 
F 
F 
  VARIABLE   
ELFORM 
DESCRIPTION 
Element  Formulation  ID  referenced  via  *SECTION_SHELL  to 
connect *ELEMENT_GENERALIZED_SHELL with the appropriate 
shell formulation.  The chosen number needs to be greater or equal
than 1000. 
NIPP 
Number of in-plane integration points. 
NMNP 
Number of nodes for this element formulation. 
IMASS 
Option for lumping of mass matrix: 
EQ.0: row sum  
EQ.1: diagonal weighting. 
FORM 
Shell formulation to be used 
EQ.0: shear  deformable  shell  theory  with  rotational  DOFs  (shell
normal evaluated at the nodes) 
EQ.1: shear  deformable  shell  theory  without  rotational  DOFs
(shell normal evaluated at the nodes) 
EQ.2: thin  shell  theory  without  rotational  DOFs  (shell  normal
evaluated at the integration points)  
EQ.3: thin  shell  theory  with  rotational  DOFs  (shell  normal
evaluated at the integration points) 
WI 
Integration weight at integration point i.
VARIABLE   
DESCRIPTION 
NKI 
Value of the shape function Nk evaluated at integration point i. 
DNKIDR 
Value of the derivative of the shape function Nk with respect to the 
local coordinate r at the integration point i (
𝜕𝑁𝑘
𝜕𝑟 ). 
DNKIDS 
Value of the derivative of the shape function Nk with respect to the 
local coordinate s at the integration point i (
𝜕𝑁𝑘
𝜕𝑠 ). 
DNKLDR 
Value of the derivative of the shape function Nk with respect to the 
local coordinate r at the nodal point l (
𝜕𝑁𝑘
𝜕𝑟 ). 
DNKLDS 
Value of the derivative of the shape function Nk with respect to the 
local coordinate s at the nodal point l (
𝜕𝑁𝑘
𝜕𝑠 ). 
D2NKIDR2 
Value  of  the  second  derivative  of  the  shape  function  Nk  with 
respect to the local coordinate r at the integration point i (
𝜕2𝑁𝑘
𝜕𝑟2 ). 
D2NKIDRDS 
Value  of  the  second  derivative  of  the  shape  function  Nk  with 
respect  to  the  local  coordinates  r  and  s  at  the  integration  point  i
𝜕2𝑁𝑘
𝜕𝑟𝜕𝑠 ). 
(
D2NKIDS2 
Value  of  the  second  derivative  of  the  shape  function  Nk  with 
respect to the local coordinate s at the integration point i (
𝜕2𝑁𝑘
𝜕𝑠2 ). 
Remarks: 
1.  For post-processing and the treatment of contact boundary conditions, the use 
of interpolation shell elements  is necessary.  
2.  The  order  of  how  to  put  in  the  data  for  the  NMNP  nodal  points  has  to  be  in 
correlation  with  the  definition  of  the  connectivity  of  the  element  in  *ELE-
MENT_GENERALIZED_SHELL.
*DEFINE_ELEMENT_GENERALIZED_SHELL 
II
III
IV
Connectivity of
Generalized-Shell Element
Generalized-Shell Element
Integration Point
*DEFINE_ELEMENT_GENERALIZED_SHELL
$#  elform 
1001 
nmnp 
9 
nipp 
4 
$# integration point 1 (i=1)
$# 
wi
1.3778659577546E-04
imass 
0 
form
$# 
dnkids
1.7098997698601E-01 3.3723996630918E+00 2.4666694616947E+00
dnkidr 
nki 
...
$# integration point 2 (i=2)
2.2045855324077E-04
5.4296436772101E-02 1.9003752917745E+00 7.8327025592051E+00
Block A
...
$# integration point 3 (i=3)
...
$# integration point 4 (i=4)
...
$# node 1 (l=1)
$# 
dnkldr 
dnklds
4.8275862102259E+00 3.5310344763662E+01
...
$# node 2 (l=2)
2.4137931051130E+00 8.8275861909156E+00
Block B
...
[...]
$# node 9 (l=9)
...
W1
k=1
k=2-9
W2
NMNP
Lines
1 (W3)+
NMNP Lines
1 (W4)+
NMNP Lines
k=1
k=2-9
NMNP
Lines
NMNP
Lines
Figure 15-31.  Example of a generalized shell formulation with *DEFINE_ELE-
MENT_GENERALIZED SHELL.
*DEFINE_ELEMENT_GENERALIZED_SOLID 
Purpose:  Define a general 3D solid formulation to be used in combination with *ELE-
MENT_GENERALIZED_SOLID.    The  objective  of  this  feature  is  to  allow  the  rapid 
prototyping  of  new  solid  element  formulations  by  adding  them  through  the  keyword 
input file. 
All necessary information, like the values of the shape functions and their derivatives at 
all integration points have to be defined via this keyword.  An example for a 18-noded 
generalized solid element with 8 integration points is given in Figure 15-31 to illustrate 
the  procedure.    The  element  formulation  ID  (called  ELFORM)  used  in  this  keyword 
needs to be greater or equal than 1000 and will be referenced through *SECTION_SOL-
ID .  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ELFORM 
NIP 
NMNP 
IMASS 
Type 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
These cards are read according to the following pseudo code: 
for i  = 1 to NIP { 
read cardA1(i) 
for k = 1 to NMNP { 
read cardA2(i,k) 
} 
} // comment: Read in NIP × (1 + NMNP) cards 
Weight Cards.  Provide weight for integration point i. 
 (Card A1)i 
Variable 
Type 
1 
2 
3 
4 
5 
6 
7 
8 
WI 
F 
Default 
none
Integration Point Shape Function Value/Derivatives Cards.  Provide the value of the 
kth shape function and its derivative at the ith integration point. 
(Card A2)ik 
Variable 
Type 
1 
2 
3 
4 
5 
6 
7 
8 
NKI 
F 
DNKIDR 
DNKIDS 
DNKIDT 
F 
F 
F 
Default 
none 
none 
none 
none 
  VARIABLE   
ELFORM 
DESCRIPTION 
Element  Formulation  ID  referenced  via  *SECTION_SOLID  to 
connect  *ELEMENT_GENERALIZED_SOLID  with  the  appropriate 
solid formulation. 
The chosen number needs to be greater or equal than 1000. 
NIP 
Number of integration points. 
NMNP 
Number of nodes for this element formulation. 
IMASS 
Option for lumping of mass matrix: 
EQ.0: row sum  
EQ.1: diagonal weighting. 
Integration weight at integration point i. 
Value of the shape function Nk evaluated at integration point i. 
WI 
NKI 
DNKIDR 
Value of the derivative of the shape function Nk with respect to the 
local coordinate r at the integration point i (
𝜕𝑁𝑘
𝜕𝑟 ). 
DNKIDS 
Value of the derivative of the shape function Nk with respect to the 
local coordinate s at the integration point i (
𝜕𝑁𝑘
𝜕𝑠 ). 
DNKIDT 
Value of the derivative of the shape function Nk with respect to the 
local coordinate t at the integration point i (
𝜕𝑁𝑘
𝜕𝑡 ).
Remarks: 
1.  For post-processing the use of interpolation solid elements  
is necessary.  
2.  The  order  of  how  to  put  in  the  data  for  the  NMNP  nodal  points  has  to  be  in 
correlation with the definition of the connectivity of the element in *ELEMENT_ 
GENERALIZED_SOLID. 
Example: 
VI
11
II
12
10
13
VII
14
VIII
III
16
15
17
IV
18
*DEFINE_ELEMENT_GENERALIZED_SOLID
$#  elform 
1001 
nmnp 
18 
nip 
8 
$# integration point 1 (i=1)
$# 
wi
1.3778659577546E-04
Connectivity of
Generalized-Solid Element
Generalized-Solid Element
Integration Point
imass
W1
k=1
k=2,18
W2
NMNP
Lines
W8
NMNP
Lines
$# 
dnkidt
1.7098997698601E-01 3.3723996630918E+00 2.4666694616947E+00 1.5327451653258E+00
dnkidr 
dnkids 
nki 
...
$# integration point 2 (i=2)
2.2045855324077E-04
5.4296436772101E-02 1.9003752917745E+00 7.8327025592051E+00 3.258715871621E+00
...
[...]
$# integration point 8 (i=8)
Block A
3.8574962585875E-04
2.6578426581235E-01 1.6258741125438E+00 2.9876495873627E+00 5.403982758392E+00
...
Figure 15-32.  Example of a generalized solid formulation with *DEFINE_EL-
EMENT_GENERALIZED_SOLID
*DEFINE_FABRIC_ASSEMBLIES 
Purpose:  Define lists of part sets to properly treat fabric bending between parts. 
Define as many cards as needed for the assemblies, using at most 8 part sets per card. 
This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SPID1 
SPID2 
SPID3 
SPID4 
SPID5 
SPID6 
SPID7 
SPID8 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
SPIDn 
Part set ID that comprises an assembly. 
Remarks: 
The materials *MAT_FABRIC and *MAT_FABRIC_MAP are equipped with an optional 
coating  feature  to  model  the  fabric’s  bending  resistance.    See  the  related  parameters 
ECOAT, SCOAT and TCOAT on these material model manual entries. 
The  default  behavior  for  these  coatings,  which  this  keyword  changes,  excludes  T-
interesections,  and,  furthermore  requires  that  all  fabric  elements  must  have  a 
consistently  oriented  normal  vector.    In  Figure  15-33,  the  left  connection  of  fabric 
elements is permitted by the default functionality while the right one is not.  However, 
with using this keyword the proper bending treatment for the right connectivity can be 
activated by adding the following input to the deck 
1 
2 
15-33. 
Figure 
Bending 
*DEFINE_FABRIC_ASSEMBLIES. 
elements belong to. 
in 
fabric, 
  The  numbers 
intended 
of
indicate  the  parts  the
use
*SET_PART_LIST 
1 
1,2 
*SET_PART_LIST 
2 
3 
*DEFINE_FABRIC_ASSEMBLIES 
1,2 
which  decouples  part  3  from  the  other  two  parts  in  terms  of  bending,  thus  creating  a 
moment free hinge along the edge between part sets 1 and 2.  Bending between parts 1 
and 2 is unaffected since these are contained in the same fabric assembly. 
For  several  instances  of  this  keyword  in  an  input  deck,  the  list  of  assemblies  is 
appended.    If  assemblies  are  defined  and  there  happens  to  be  fabric  parts  that  do  not 
belong  to  any  of  the  specified  assemblies,  then  these  parts  are  collected  in  a  separate 
unlisted  assembly.    The  restriction  on  consistent  normal  vectors  and  on  having  no  T-
intersections applies to all elements within an assembly.
*DEFINE_FILTER 
Purpose:  Define a general purpose filter, currently used by this option: 
SENSOR_SWITCH 
The input in this section consists of two cards: 
  Card 1 
Variable 
1 
ID 
Type 
I 
2 
3 
4 
5 
6 
7 
8 
Title 
A70 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Type 
Type 
Data1 
Data2 
Data3 
Data4 
Data5 
Data6 
Data7 
Type 
A10 
  VARIABLE   
DESCRIPTION
ID 
Title 
Type 
Identification number. 
Title for this filter. 
One  of 
CONTINUOUS, or CHAIN 
the  3  currently  defined 
filter 
types:  DISCRETE,
Data1-7 
Filter type specific data, which determines what the filter does. 
Filter Types: 
FILTER 
DISCRETE 
DESCRIPTION
The  discrete  filter  operates  on  a  fixed  number  of  values  of  the
input data.  The first data field is an A10 character field, which
gives the type of operation the filter performs:  MIN, MAX, and
AVG are the available options.  The second data field is an I10 
field,  giving  the  number  of  input  values  over  which  the
minimum, maximum, or average is computed.
CONTINUOUS 
CHAIN 
*DEFINE 
DESCRIPTION
Similar  to  the  DISCRETE  filter,  except  that  it  operates  over  a
fixed time interval.  The first data field is exactly the same as for
the  DISCRETE  option.    The  second  data  field  is  an  F10  field,
indicating  the  duration  of  the  filter.    For  example,  if  AVG  is
given,  and  the  duration  is  set  to  0.1,  a  running  timestep
weighted  average  is  computed  over  the  last  0.1  time  of  the
simulation. 
Here, data fields 1-7 are all I10 fields, and give the IDs of a list 
of other filters (including other CHAIN filters, if desired), each
of which will be applied in order.  So the raw data is fed to the
filter indicated by  Data1.  The output of that is fed to the next 
filter,  and  so  on,  with  up  to  7  filters  in  the  chain.    List  only  as
many filters as you need.
*DEFINE_FORMING_BLANKMESH 
Purpose:  This keyword, together with keyword *ELEMENT_BLANKING, enable mesh 
generation  for  a  sheet  metal  blank.    This  keyword  is  renamed  from  the  previous 
keyword  *CONTROL_FORMING_BLANKMESH.    The  keyword  *DEFINE_CURVE_-
TRIM_NEW  can  be  coupled  with  this  keyword  to  define  a  blank  with  a  complex 
periphery and a number of inner hole cutouts.   
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IDMSH 
ELENG 
XLENG 
YLENG 
ANGLEX  NPLANE 
CID 
Type 
I 
F 
F 
F 
F 
Default 
none 
0.0 
0.0 
0.0 
0.0 
  Card 2 
1 
2 
3 
4 
5 
I 
1 
6 
I 
0 
7 
8 
Variable 
PIDBK 
NID 
EID 
XCENT 
YCENT 
ZCENT 
XSHIFT 
YSHIFT 
Type 
Default 
I 
1 
I 
1 
I 
1 
F 
F 
F 
F 
F 
0.0 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
IDMSH 
ID of the blankmesh (not the blank PID); must be unique. 
ELENG 
Element edge length. 
XLENG 
YLENG 
ANGLEX 
Length  of  the  rectangular  blank  along  X-axis  in  the  coordinate 
system (CID) defined. 
Length  of  the  rectangular  blank  along  Y-axis  in  the  coordinate 
system (CID) defined. 
An angle defined about Z-axis of the CID specified, starting from 
the  X-axis  as  the  zero  degree,  to  rotate  the  blank  and  the
orientation of the mesh to be generated.  The sign of the rotation 
angle follows the right hand rule.  See Remark 3.
VARIABLE   
NPLANE 
DESCRIPTION
Plane  in  which  a  flat  blank  to  be  generated,  in  reference  to  the
coordinate system defined (CID): 
EQ.0 or 1: XY-plane (default) 
EQ.2: 
EQ.3: 
XZ-plane 
YZ-plane 
CID 
ID of the local coordinate system, defined by *DEFINE_COORDI-
NATE_SYSTEM.    Default  is  0  representing  global  coordinate
system. 
PIDBK 
Part ID of the blank, as defined by *PART. 
NID 
EID 
Starting node ID of the blank to be generated. 
Starting element ID of the blank to be generated. 
XCENT 
X-coordinate of the center of the blank. 
YCENT 
Y-coordinate of the center of the blank. 
ZCENT 
Z-coordinate of the center of the blank. 
XSHIFT 
YSHIFT 
Blank  shifting  distance  in  X-axis  in  coordinate  system  defined 
(CID).  
Blank  shifting  distance  in  Y-axis  in  coordinate  system  defined 
(CID). 
About the keyword: 
A rectangular blank is defined and meshed, which can be trimmed with IGES curves to 
a  desired  periphery  and  inner  cutouts.    This  keyword  is  used  in  conjunction  with 
keyword *ELEMENT_BLANKING.  The blank outlines and inner holes can be defined 
using keyword *DEFINE_CURVE_TRIM_NEW. 
Application example: 
A  partial  keyword  example  of  generating  a  flat  blank  with  PID  1  is  provided  blow.  
Referring  to  Figure  15-34,  the  blank  mesh  is  to  be  generated  in  XY  plane  in  a  global 
coordinate  system,  with  an  average  element  edge  length  of  12  mm  and  a  blank 
dimension of 1100.0 x 1050.0 mm, with node and element ID starting at 8000, and with 
the  center  of  the  blank  in  the  global  origin.    The  blank  is  to  be  trimmed  out  with  an
inner  cut-out  hole,  given  by  the  IGES  file  innerholes.iges.    Blank  outer  line  is  defined 
with an IGES file outerlines.iges. Both IGES files are used to trim the rectangular blank 
using  keyword  *DEFINE_CURVE_TRIM_NEW,  where  the  variable  TFLG  is  used  to 
indicate  whether  it  is  an  inside  or  outside  trim.    The  blank  generated  for  example  is 
shown in Figure 15-35. 
*KEYWORD 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*CONTROL_TERMINATION 
$#  endtim 
     0.000 
*CONTROL_FORMING_BLANKMESH 
$    IDMSH     ELENG     XLENG     YLENG    ANGLEX    NPLANE       CID 
         3     12.00   1100.00     895.0       0.0         0         0 
$    PIDBK       NID       EID     XCENT     YCENT     ZCENT    XSHIFT    YSHIFT 
         1      8000      8000      
*ELEMENT_BLANKING 
$#    psid 
         1 
*DEFINE_CURVE_TRIM_NEW 
$#    tcid    tctype      TFLG      TDIR     TCTOL      TOLN    NSEED1    NSEED2 
     11111         2         1         0  0.250000  1.000000  
innerholes.iges 
*DEFINE_CURVE_TRIM_NEW 
$#    tcid    tctype      TFLG      TDIR     TCTOL      TOLN    NSEED1    NSEED2 
     11112         2        -1         0  0.250000  1.000000  
outerlines.iges 
*CONTROL_SHELL 
...... 
*CONTROL_SOLUTION 
......  
*DATABASE_BINARY_D3PLOT 
...... 
*DATABASE_EXTENT_BINARY 
...... 
*SET_PART_list 
1 
1 
*PART 
Blank                                                                            
$#     pid     secid       mid  
         1         1         1  
*SECTION_SHELL 
$#   secid    elform      shrf       nip     propt   qr/irid     icomp     setyp 
         1        16  0.833000         7         1         0         0         0 
$#      t1        t2        t3        t4      nloc     marea      idof    edgset 
  1.500000  1.500000  1.500000  1.500000     0.000     0.000     0.000         0 
*MAT_037 
$#     mid        ro         e        pr      sigy      etan         r     hlcid 
         1 7.9000E-9 2.0700E+5  0.300000 253.25900     0.000  1.408000     90903 
*DEFINE_CURVE 
     90903      
253.2590027 
...... 
           0.9898300         616.7999878 
*INTERFACE_SPRINGBACK_LSDYNA 
$#    psid      nshv 
         1      1000 
*END
The  blank  and  mesh  orientation  can  be  rotated  about  Z-axis  defined.    Following  the 
right hand rule, the blank in this case is rotated about Z-axis for a positive 30°, as shown 
in Figure 15-35, with the angle of 0° aligned with X-axis. 
Inner  hole  and  outer  periphery  can  also  be  trimmed  using  the  NSEEDs  variables  in 
keyword *DEFINE_CURVE_TRIM_NEW. 
Revision information: 
This  feature  is  available  in  LS-DYNA  Revision  59165  or  later  releases.    The  keyword 
name change from *CONTROL… to *DEFINE… started in Revision 69074.  The variable 
NPLANE is implemented in Revision 69128 and later releases.
Blank outlines
(outlines.iges)
Inner cutout
(innerhole.iges)
Regutangular blank of  1100.0x1050.0mm
Figure 15-34.  Initial input for a blank meshing.
30 deg. 
Figure 15-35.  Resulting blank mesh.
*DEFINE_FORMING_CLAMP 
Purpose:  This keyword simplifies the process definition during a clamping simulation, 
and works as a macro serving as a placeholder for the combination of cards needed to 
model  a  clamping  process  such  as  those  that  are  commonly  used  in  sheet  metal 
forming.  A related keyword includes *DEFINE_FORMING_CONTACT. 
Define Clamp Card.  Define one card for each clamp set.  Include as many cards in the 
following format as desired.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
Variable 
CLP1 
CLP2 
VID 
GAP 
Type 
I 
I 
I 
F 
5 
AT 
F 
6 
DT 
F 
7 
8 
Default 
none 
none 
none 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
CLP1 
CLP2 
Part  ID  of  a  moving  rigid  body  clamp,  defined  by  *PART  and
*MAT_020 (*MAT_RIGID). 
Part  ID  of  a  fixed  rigid  body  clamp,  defined  by  *PART  and
*MAT_020.  This is sometimes called “net pad”. 
VID 
Define CLP1 moving direction: 
GT.0: Vector  ID  from  *DEFINE_VECTOR,  specifying  the 
moving direction of CLP1 
LT.0:  Absolute value is a node ID, whose normal vector will be 
used to define the moving direction of CLP1. 
Final  desired  distance  between  CLP1  and  CLP2  at  the  end  of
clamping. 
Begin time for CLP1’s move. 
Duration of CLP1’s move. 
GAP 
AT 
DT
*DEFINE 
One typical application of this keyword is to estimate springback during the clamping 
of a formed panel on a checking fixture.  Net pads (lower fixed regular or square pads) 
of  a  few  millimeters  thick  are  placed  according  to  GD&T  (Geometry  Dimensioning  and 
Tolerancing) requirements on a support platform, typically taking shape of the nominal 
product.    Each  net  pad  (CLP2,  see  Figure  15-36)  has  a  corresponding  moving  clamp 
(CLP1). 
The movable clamp (CLP1) is initially open so that the formed panel can be loaded onto 
the  net  pads.    Four-way  and  two-way  position  gaging  pins  are  used  to  initially  locate 
and  load  the  panel  in  the  fixture,  before  CLP1  is  moved  to  close  with  the  net  pad 
(CLP2).  A white light scan is then performed on the panel and scan data is processed to 
ascertain  the  degree  of  panel  conformance  to  the  required  nominal  shape.    Even  with 
the  clamps  fully  closed,  some  severely  distorted  panels  will  significantly  deviate  from 
the nominal shape when the residual stresses from the forming process are too great. 
Although, unrelated to this keyword another common method to  determine the panel 
springback amount is the free state check which involves a white light scan on the panel 
secured on a platform but with no additional forces (clamps – CLP1s) applied to deform 
the panel (to the net pads CLP2s, for example).  LS-DYNA can model both methods and 
job  setups  can  be  easily  done  by  selecting  Implicit  Static Flanging process  in  LS-PrePost 
4.2’s 
eZ-Setup 
(http://ftp.lstc.com/anonymous/outgoing/lsprepost/4.2/win64/).  Furthermore, once 
springback has been determined die compensation (*INTERFACE_COMPENSATION_-
NEW)  can  then  be  performed  to  minimize  or  eliminate  the  springback;  the  resulting 
compensated die shapes can be surfaced, re-machined to produce panels that are within 
dimensional tolerance. 
Application 
Forming 
Metal 
/ 
Since the clamp is, typically, modelled with a much coarser mesh than that on a blank, 
*CONTACT_FORMING_SURFACE_TO_SURFACE  should  be  used.    Rotating-type  of 
clamps are currently not supported. 
Application example: 
A  partial  keyword  example  of  using  the  feature  is  listed  below.    Referring  to  Figure 
15-36, the drawn and trimmed blank is positioned between the clamps CLP1 and CLP2.  
The implicit termination “time” is  set at 1.0, with a stepping size  of 0.25, for a total of 
four steps – two steps each for the two CLP1.  With the original blank thickness of 1.0 
mm,  the  CLP1s  are  set  to  close  with  the  lower  CLP2s  at  “time”  of  1.0,  leaving  a  total 
GAP  of  1.02  mm.    Note  the  VIDs  are  defined  as  “-46980”,  indicating  that  the  moving 
clamps (CLP1) will move in the normal direction defined by Node #46980.  The contact 
definition 
using 
between 
*DEFINE_FORMING_CONTACT. 
defined 
clamps 
panel 
and 
the 
the 
are
*KEYWORD 
*INCLUDE 
./trimmed.dynain 
./nets.k 
*CONTROL_TERMINATION 
1.0 
*CONTROL_IMPLICIT_forming 
1 
*control_implicit_general 
1,0.25 
*CONTROL_SHELL 
⋮  
*DATABASE_EXTEND_BINARY 
⋮  
*PART 
Blank 
$      PID     SECID       MID 
         1         1         1 
Clamp1 
2,2,2 
Clamp2 
3,2,3 
Clamp3 
4,2,2 
Clamp4 
5,2,3 
*MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLASTIC 
$      MID        RO         E        PR      SIGY      ETAN         R     HLCID 
         1 2.700E-09 12.00E+04      0.28       0.0       0.0     0.672         2 
*MAT_RIGID 
$#     mid        ro         e        pr         n    couple         m     alias 
         2 7.8500E-9 2.1000E+5  0.300000  
$#     cmo      con1      con2 
  1.000000         7         7 
$# lco or a1      a2        a3        v1        v2        v3 
     0.000     0.000     0.000     0.000     0.000     0.000 
*MAT_RIGID 
$#     mid        ro         e        pr         n    couple         m     alias 
         3 7.8500E-9 2.1000E+5  0.300000  
$#     cmo      con1      con2 
  1.000000         4         7 
$# lco or a1      a2        a3        v1        v2        v3 
*SETION_SHELL 
1,16,,7 
1.0,1.0,1.0,1.0 
*LOAD_BODY_Z 
      9997       1.0 
*DEFINE_CURVE 
      9997 
              0.0000           9810.0000 
              1.0000           9810.0000 
*DEFINE_FORMING_CLAMP 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
$     CLP1      CLP2       VID       GAP        AT        DT 
         3         2    -46980      1.02       0.0       0.5 
         5         4    -46980      1.02       0.5       0.5 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*DEFINE_FORMING_CONTACT 
$      IPS       IPM        FS    ONEWAY 
         1         2     0.125         1 
         1         3     0.125         1 
         1         4     0.125         1 
         1         5     0.125         1 
*END
Note with this keyword, formed panel needs to be pre-positioned properly with respect 
to  the  clamps  by  users,  and  auto-position  (*CONTROL_FORMING_AUTOPOSITION) 
cannot  be  used.    Furthermore,  prescribed  motions  and  clamp  motion  curves  do  not 
need to be defined for the clamps. 
Revision information: 
This  feature  is  available  starting  in  double  precision  LS-DYNA  Revision  99007  for 
implicit static only.
Element normals of 
the moving clamps
Element normals 
of the net pads
Initial position
(side view); t=0.0
First clamp moving down half-
way; panel springs back; t=0.25
First clamp completes 
moving; t=0.50
GAP 
Second clamp moving 
down half-way; t=0.75
Second clamp completes 
moving (fully clamped); t=1.0
Formed & trimmed 
blank (before 
springback)
Fixed net pads
(CLP2)
Node 46980 
Second moving 
clamp (CLP1) 
First moving clamp
(CLP1) 
Initial position (iso-view);
t=0.0
Fully clamped position (iso-view)
t=1.0
 Figure 15-36.  Variable definitions and an example of using the negative VID.
*DEFINE 
Purpose:  This keyword works as macro for the FORMING_(ONE_WAY)_SURFACE_-
TO_SURFACE  keyword.    It  adds  one  contact  definition  to  the  model  per  data  card.  
Each data card consists of a reduced set of FIELDS compared with the full *CONTACT 
keyword.    The  omitted  fields  take  their  default  values.    A  related  keyword  includes 
*DEFINE_FORMING_CLAMP. 
Define  Contact  Card.    Define  one  card  for  each  contact  interface.    Define  as  many 
cards in the following format as desired.  The input ends at the next keyword (“*”) card.
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IPS 
IPM 
FS 
ONEWAY 
Type 
I 
I 
F 
Default 
none 
none 
none 
I 
0 
  VARIABLE   
DESCRIPTION
IPS 
IPM 
Part  ID  of  a  slave  sliding  member,  typically  a  deformable  sheet
metal blank. 
Part ID of a master sliding member, typically a tool or die defined
as a rigid body. 
Deformable blank
PID 1
Fixed net pad 
PID 5
Clamp PID 2 
Fixed net pad 
PID 4
Clamp PID 3 
Figure 15-37.  Define contact interfaces.
*DEFINE_FORMING_CONTACT 
DESCRIPTION
FS 
Coulomb friction coefficient. 
ONEWAY 
Define FORMING contact type: 
EQ.0: The  contact  is  FORMING_ONE_WAY_SURFACE_TO_-
SURFACE. 
EQ.1: The contact is FORMING_SURFACE_TO_SURFACE. 
Application example: 
A  partial  keyword  example  of  defining  contact  between  a  deformable  part  and  two 
pairs  of  clamps  is  given  below.    In  Figure  15-37,  a  blank  PID  of  1  is  defined  to  have 
FORMING_SURFACE_TO_SURFACE contact with rigid body clamps of PID of 2, 3, 4, 
and  5,  with  coefficient  of  frictions  for  each  interface  as  0.125,  0.100,  0.125,  and  0.100, 
respectively.  Only a total of four lines are needed to define four contact interfaces, as 
opposed to at least three cards for each interface. 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*DEFINE_FORMING_CONTACT 
$      IPS       IPM        FS    ONEWAY 
         1         2     0.125         1 
         1         3     0.100         1 
         1         4     0.125         1 
         1         5     0.100         1 
Revision information: 
This feature is available starting in LS-DYNA Revision 98988.
*DEFINE 
Purpose:  Define friction coefficients between parts for use in the contact options: 
SINGLE_SURFACE, 
AIRBAG_SINGLE_SURFACE, 
AUTOMATIC_GENERAL, 
AUTOMATIC_SINGLE_SURFACE, 
AUTOMATIC_SINGLE_SURFACE_MORTAR, 
AUTOMATIC_NODES_TO_SURFACE, 
AUTOMATIC_SURFACE_TO_SURFACE, 
AUTOMATIC_SURFACE_TO_SURFACE_MORTAR, 
AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE, 
ERODING_SINGLE_SURFACE. 
The  input  in  this  section  continues  until  then  next  “*”  card  is  encountered.    Default 
friction values are used for any part ID pair that is not defined. 
The coefficient tables specified by the following cards are activated when FS   is  set  to  -2.0.    This  feature  overrides  the  coefficients  defined  in 
*PART_CONTACT (which are turned on only when FS is set to -1.0). 
When  only  one  friction  table  is  defined,  it  is  used  for  all  contacts  having  FS  set  to  -2.  
Otherwise,  for  each  contact  with  FS  equal  to  -2,  the  keyword  reader  assigns  a  table  to 
each *CONTACT by matching the value of FD from *CONTACT with an ID from Card 
1 below.  Failure to match FD to an ID causes error termination. 
  Card 1 
Variable 
Type 
Default 
1 
ID 
I 
0 
2 
3 
4 
5 
6 
7 
8 
FS_D 
FD_D 
DC_D 
VC_D 
F 
F 
F 
F 
0.0 
0.0 
0.0 
0.0
Friction  ij  card.    Sets  the  friction  coefficients  between  parts  i  and  j.    Add  as  many  of 
these  cards  to  the  deck  as  necessary.    The  next  keyword  (“*”)  card  terminates  the 
friction definition. 
Card 2… 
1 
Variable 
PIDi 
2 
PIDj 
3 
FSij 
4 
FDij 
5 
DCij 
6 
7 
8 
VCij 
PTYPEi 
PTYPEj 
Type 
I 
I 
F 
F 
F 
F 
A 
A 
Default 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
ID 
FS_D 
FD_D 
DC_D 
Identification number.  Only one table is allowed. 
Default  value  of  the  static  coefficient  of  friction.    The  frictional
coefficient is assumed to dependend on the relative velocity 𝑣rel of 
the surfaces in contact, 
𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣. 
Default values are used when part pair are undefined.  For mortar
contact 𝜇𝑐 = FS, i.e., dynamic effects are ignored. 
Default value of the dynamic coefficient of friction.  The frictional
coefficient is assumed to depended on the relative velocity 𝑣rel of 
the surfaces in contact, 
𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣re𝑙∣. 
Default values are used when part pair are undefined.  For mortar
contact 𝜇𝑐 = FS, i.e., dynamic effects are ignored. 
Default value of the exponential decay coefficient.  The frictional
coefficient is assumed to be depend on the relative velocity 𝑣rel of 
the surfaces in contact, 
𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣. 
Default values are used when part pair are undefined.  For mortar
contact 𝜇𝑐 = FS, i.e., dynamic effects are ignored.
VARIABLE   
VC_D 
DESCRIPTION
Default  value  of  the  coefficient  for  viscous  friction.    This  is
necessary  to  limit  the  friction  force  to  a  maximum.    A  limiting
force is computed 
𝐹lim = VC × 𝐴cont, 
where  𝐴cont  is  the  area  of  the  segment  contacted  by  the  node  in 
contact.    The  suggested  value  for VC  is  to  use  the  yield  stress  in 
  where  σo  is  the  yield  stress  of  the  contacted 
shear  VC =
𝜎𝑜
√3
material.  Default values are used when part pair are undefined. 
PIDi 
PIDj 
FSij 
FDij 
DCij 
VCij 
PTYPEi, 
PTYPEj 
Part, or part set, ID i. 
Part, or part set, ID j. 
Static coefficient of friction between parts i and j. 
Dynamic coefficient of friction between parts i and j. 
Exponential decay coefficient between parts i and j. 
Viscous friction between parts i and j. 
EQ.“PSET”: when PTYPEi or PTYPEj refers to a *SET_PART.
*DEFINE_FRICTION_ORIENTATION 
Purpose:  This keyword allows for definition of different coefficients of friction (COF) in 
specific directions, specified using a vector and angles in degree.  In addition, COF can 
be  scaled  according  to  the  amount  of  pressure  generated  in  the  contact  interface.  This 
feature is intended for use with FORMING_ONE_WAY type of contacts.  This feature is 
developed jointly with the Ford Motor Company. 
  Card 1 
1 
2 
3 
Variable 
PID 
LCID 
LCIDP 
Type 
I 
Default 
none 
I 
0 
I 
0 
7 
8 
4 
V1 
F 
5 
V2 
F 
6 
V3 
F 
0.0 
0.0 
0.0 
DESCRIPTION
  VARIABLE   
PID 
Part  ID  to  which  directional  and  pressure-sensitive  COF  is  to  be 
applied.  See *PART. 
LCID 
ID of the load curve defining COF vs.  orientation in degree. 
LCIDP 
ID of the load curve defining COF scale factor vs.  pressure. 
V1 
V2 
V3 
Vector  components  of  vector  V  defining  zero-degree  (rolling) 
direction. 
Vector  components  of  vector  V  defining  zero-degree  (rolling) 
direction. 
Vector  components  of  vector  V  defining  zero-degree  (rolling) 
direction. 
The assumption: 
Load  curves  LCID  and  LCIDP  are  not  extrapolated  beyond  what  are  defined.    It  is 
recommended  that  the  definition  is  specified  for  the  complete  range  of  angle  and 
pressure  expected.    One  edge  of  all  elements  on  the  sheet  metal  blank  must  align 
initially with the vector defined by V1, V2, and V3.
Application example: 
The  following  is  a  partial  keyword  input  of  using  this  feature  to  define  directional 
frictions and pressure-sensitive COF scale factor. 
*DEFINE_FRICTION_ORIENTATION 
$      PID      LCID     LCIDP        V1        V2        V3 
         1        15        16       1.0        0.        0. 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ define COF vs.  orientation angle 
*DEFINE_CURVE 
15 
0.0, 0.3 
90.0, 0.0 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ define COF scale factor vs.  pressure 
*DEFINE_CURVE 
16 
0.1, 0.3 
0.2, 0.3 
0.3, 0.3 
0.4, 0.2 
0.5, 0.5 
0.6, 0.4 
Referring to Figure 15-38, a deformable blank is clamped with 1000N of force between 
two  rigid  plates  and  is  pulled  along  the  direction  of  X-axis  for  90  mm  using 
displacement control.  Initial and final positions of the blank are shown in Figure 15-39.  
The  normal  force  is  recovered  from  RCFORC  file,  as  shown  in  Figure  15-40,  which 
agrees with what is applied.  Frictional force (pulling force) in X-direction is plotted as 
89N, shown in Figure 15-41.  A hand calculation from the input verifies this result: 
[clamping force]
⏟⏟⏟⏟⏟⏟⏟⏟⏟
1000𝑁
× [𝑥-dir coefficient]
⏟⏟⏟⏟⏟⏟⏟⏟⏟
0.3
× [coefficient scale factor at 0.27 pressure]
⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟
0.3
= 90𝑁 
The  interface  pressure  can  be  output  from  an  LS-DYNA  run  when  ‘S = filename’  is 
included in the command line.  The binary output can be viewed from LS-PrePost4.0. 
The  element  directions  are  automatically  aligned  with  the  vector  V.    The  left  side  of 
Figure  15-42  shows  the  element  directions  of  the  incoming  sheet  blank.    The  keyword 
will  re-orient  the  element  directions  based  on  the  vector  V  specified,  which  has  the 
component of [1.0, 0.0, 0.0] in this case.  The re-oriented element directions for the blank 
are shown on the right side of the Figure. 
Following  the  numeric  directions  provided in  Figure  15-43,  LS-PrePost4.0  can  be  used 
to check the element directions of a sheet blank.  
This feature is generally developed for use with FORMING_ONE_WAY type of contact 
in SMP.  However, this keyword can be used in combination with *CONTACT_FORM-
ING_ONE_WAY_SURFACE  TO_SURFACE_ORTHO_FRICTION,  and  in  fact,  it  can 
only  be  used  in  this  manner  if  running  MPP.    In this  combination,  the  variables  LCID 
and  LCIDP  are  overridden  by  friction  factor  input  in  ORTHO_FRICTION,  while  the
vector  [V1,  V2,  V3]  defines  the  first  orthogonal  direction.    It  furthermore  allows  the 
convenience  of  SSID  and  MSID  in  *CONTACT  being  input  as  part  set  IDs  (when 
SSTYP/MSTYP = 2), in which case the segments sets necessary for ORTHO_FRICTION 
are  generated  automatically  with  orientation  according  to  the  vectors  defined  by  [V1, 
V2,  V3].     The  part  set  ID  input  option  is  typically  used  by  metal  forming  users.    A 
detailed keyword example is shown in Figure 15-44. 
Revision information: 
This  feature  is  available  in  LS-DYNA  Revision  60275  and  later  releases  for  SMP.    It 
works  with  MPP  with  one  way  forming  type  of  contact  with  ORTHO_FRICTION 
starting  from  Rev  73226.  In  addition,  it  works  with  SMOOTH  contact  option  starting 
from Revision 69631.
1000N applied on upper rigid plate, about 0.27 N/mm2
of pressure on the deformable blank.
Lower rigid plate fixed, 
of size 169 x 169mm
Pull 90mm in X on each node along 
the edge of a deformable blank of 
size 61.25 x 61.25mm)
Figure [15-38].  Boundary and loading conditions of a small test model. 
max=90.0045, at node #149
X-displacement
(mm)
Final position
Initial position
90
81
72
63
54
45
36
27
18
Figure [15-39].  Initial and final position of the blank.
-0.2
-0.4
-0.5
-1
)
(
-
-1.2
0.05
0.1
0.15
Time (sec)
Figure [15-40].  Normal force from RCFORC file. 
)
(
-
100
80
60
40
20
0.05
0.1
0.15
Time (sec)
Figure [15-41].  Pulling force (frictional force) from RCFORC file.
Figure [15-42].  Element directions (N1-N2) of an incoming sheet blank (left)
and directions after re-orientation. 
Identify
Element
Particle
Node
Part
CNRB
Shell
Solid
Beam
Seat.
SPH
Mass
Disc.
DiscSph.
Iner.
Nurbs
Tshel
AnyE
Key in xyz coord
Show Results
Elem Dir
Mat Dir
No ID
AirbagR
Show Popup
Echo
Ident
RefGeo
Find
Curve
Blank
Surf
MovCop
Solid
Offset
GeoTol
Transf
Mesh
Normal
Model
DetEle
EleTol
DupNod
Post
NodEdit
MFPre
Part Name
EleEdit
MFPost
Measur
Favor1
Clear Node
Clear Elem
Clear All
Clear Node
Clear Elem
Clear All
Clear Node
Clear Elem
Clear All
ByNode
ByElem
ByPart
ByGpart
BySubsys
BySET
ByEdge
ByPath
BySegm
ByCurve
BySurf
Total identified nodes:
Total identified elems:
Total identified parts:
Total identified particles:
Total identified CNRBs:
Clear Node
Clear Part
Clear Elem
Clear CNRB
Clear All
Done
Sel. Elem. (0)
Pick
Area
Poly
Sel1
Sphe
Box
Prox
Circ
Frin
Plan
In
Out
Add
Rm
ID
Type
any
Label selection 
3DSurf
Figure  [15-43].    Checking  element  directions  (N1-N2)  by  part  using  LS-
PrePost4.0.
*DEFINE_FRICTION_ORIENTATION
$      PID      LCID      LCIDP                V1            V2          V3
            1,,,                                      1.0          0.0          0.0
*CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ORTHO_FRICTION
$    SSID      MSID      SSTYP      MSTYP
            1,          3,            2,            2
$        FS          FD            DC            VC
      1.25,      0.0,                      20.0
$      SFS      SFM
        0.0,    0.0
$FS1_S,  FD1_S,  DC1_S,  VC1_S,  LC1_S,  OACS_S,  LCFS,  LCPS
      0.3,      0.0,      0.0,      0.0,,          ,            1,      15,      16
$FS2_S,  FD2_S,  DC2_S,  VC2_S,  LC2_S
      0.1,      0.0,      0.0,      0.0
$FS1_M,  FD1_M    DC1_M,  VC1_M,  LC1_M,  OACS_M,  LCMS,  LCPM
      0.3,      0.0,      0.0,      0.0,            ,            0,      15,      16
$FS2_M,  FD2_M,  DC2_M,  VC2_M,  LC2_M
      0.1,      0.0,      0.0,      0.0
*DEFINE_CURVE
$  LCFS,  define  COF  vs.  angle  based  on  1st  orthogonal  direction
15
0.00,0.3
45.0,0.2
90.0,0.1
*DEFINE_CURVE
$  LCPS,  define  COF  scale  factor  vs.  pressure
16
0.0,0.0
0.3,0.3
0.5,0.5
Use this keyword/vector to define rolling direction
Use *Set_part_list
FS ignored if ORTHO_FRICTION is 
present
FS1_S, LC1_S ignored if LCFS, LCPS are 
defined:
LCFS: COF vs. Angle;  
LCPS: COF scale factor vs. Pressure.
FS1_M, LC1_M ignored if LCFM, LCPM 
are defined
1st Orthogonal direction follows slave segment  
orientation, as defined by ‘a1’ in *SET_SEGMENT; 
Ignored when defined with 
*DEFINE_FRICTION_ORIENTATION.
1st Orthogonal direction follows slave segment  
orientation, as defined by ‘a1’ in *SET_SEGMENT; 
Ignored when defined with 
*DEFINE_FRICTION_ORIENTATION.
  Figure [15-44].  Use of this keyword with _ORTHO_FRICTION for MPP.
*DEFINE 
Purpose:    Define  a  function  that  can  be  referenced  by  a  limited  number  of  keyword 
options.    The  function  arguments  are  different  for  each  keyword  that  references  *DE-
FINE_FUNCTION.    Unless  stated  otherwise,  all  the  listed  argument(s)  in  their  correct 
order  must  be  included  in  the  argument  list.    Some  usages  of  *DEFINE_FUNCTION 
allow  random  ordering  of  arguments  and  argument  dropouts.    See  the  individual 
keywords for the correct format.  Some examples are shown below.  
The TITLE option is not allowed with *DEFINE_FUNCTION.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FID 
Type 
I 
HEADING 
A70 
Function Cards.  Insert as many cards as needed.  These cards are combined to form a 
single line of input.  The next keyword (“*”) card terminates this input. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
  VARIABLE   
FID 
FUNCTION 
A80 
DESCRIPTION
Function  ID.    Functions,  tables  ,  and  load 
curves may not share common ID's.  A unique number has to be
defined. 
HEADING 
An optional descriptive heading. 
FUNCTION 
Arithmetic  expression  involving  a  combination  of  independent
variables  and  other  functions,  i.e.,  “f(a,b,c)=a*2+b*c+sqrt(a*c)” 
where  a,  b,  and  c  are  the  independent  variables.    The  function
name,  “f(a,b,c)”,  must  be  unique  since  other  functions  can  then 
use 
example,
“g(a,b,c,d)=f(a,b,c)**2+d”.  In this example, two *DEFINE_FUNC-
TION definitions are needed to define functions f and g. 
reference 
function. 
and 
this 
For
*DEFINE_FUNCTION 
The following examples serve only as an illustration of syntax. 
Unlike  *DEFINE_CURVE  and  *DEFINE_CURVE_FUNCTION,  *DEFINE_FUNCTION 
is always active in dynamic relaxation phase. 
Example 1: 
Prescribe sinusoidal 𝑥-velocity and 𝑧-velocity for some nodes. 
*BOUNDARY_PRESCRIBED_MOTION_SET 
$#    nsid       dof       vad      lcid        sf       
         1         1         0         1 
         1         3         0         2 
*DEFINE_FUNCTION 
1,x-velo 
x(t)=1000*sin(100*t) 
*DEFINE_FUNCTION 
2,z-velo 
a(t)=x(t)+200 
Example 2: 
Ramp up a hydrostatic pressure on a submerged surface. 
*comment 
units: mks 
Apply a hydrostatic pressure ramped up over a finite time = trise. 
pressure on segment = rho * grav * depth of water 
where depth of water is refy - y-coordinate of segment 
and refy is the y-coordinate of the water surface 
*DEFINE_FUNCTION 
10 
float  hpres(float  t,  float  x,  float  y,  float  z,  float  x0,  float  y0, 
float z0) 
{ 
  float  fac, trise, refy, rho, grav; 
  trise = 0.1; refy = 0.5; rho = 1000.; grav = 9.81; 
  fac = 1.0; 
  if(t<=trise) fac = t/trise; 
  return fac*rho*grav*(refy-y); 
} 
*LOAD_SEGMENT_SET 
1,10  
Example  2  illustrates  that  a  programming  language  resembling  C  can  be  used  in 
defining a function.  Before a variable or function is used, its type must be declared; that 
is the purpose of "float" (i.e., a real variable rather than integer type) appearing before
those  entities.    The  braces  indicate  the  beginning  and  end  of  the  function  being 
programmed.  Semicolons must appear after each statement but several statements may 
appear  on  a  single  line.    Please  refer  to  a  C  programming  guide  for  more  detailed 
information.
*DEFINE_FUNCTION_TABULATED 
Purpose:    Define  a  function  of  one  variable  using  two  columns  of  input  data  (in  the 
manner  of  *DEFINE_CURVE)  that  can  be  referenced  by  a  limited  number  of  keyword 
options or by other functions defined via *DEFINE_FUNCTION.   
The TITLE option is not allowed with *DEFINE_FUNCTION_TABULATED. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FID 
Type 
I 
HEADING 
A70 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
FUNCTION 
A80 
Point Cards.  Put one pair of points per card (2E20.0).  Add as many cards as necessary. 
Input is terminated when a keyword (“*”) card is found.  
  Cards 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
A1 
F 
Default 
0.0 
O1 
F 
0.0 
  VARIABLE   
FID 
DESCRIPTION
Function  ID.    Functions,  tables  ,  and  load 
curves may not share common ID's.  A unique number has to be
defined. 
HEADING 
An optional descriptive heading. 
FUNCTION 
Function name.
VARIABLE   
DESCRIPTION
A1, A2, … 
Abscissa values. 
O1, O2, … 
Ordinate (function) values. 
Example: 
*BOUNDARY_PRESCRIBED_MOTION_SET 
$  function 300 prescribes z-acceleration of node set 1000 
1000,3,1,300 
*DEFINE_FUNCTION_TABULATED 
201 
tabfunc 
0., 200 
0.03, 2000. 
1.0, 2000. 
*DEFINE_FUNCTION 
300 
a(t)=tabfunc(t)*t 
$$  following function is equivalent to one above for t < 0.03 
$ a(t)=(200.  + 60000.*t)*t
*DEFINE_GROUND_MOTION 
Purpose:    Define  an  earthquake  ground  motion  history  using  ground  motion  records 
provided as load curves, for use in conjunction with *LOAD_SEISMIC_SSI for dynamic 
earthquake analysis including nonlinear soil-structure interaction. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
GMID 
ALCID 
VLCID 
Type 
I 
I 
Default 
none 
none 
I 
0 
  VARIABLE   
DESCRIPTION
GMID 
Ground motion ID.  A unique number has to be defined. 
ALCID 
Load curve ID of ground acceleration history. 
VLCID 
Load curve ID of ground velocity history. 
Remarks: 
1.  Earthquake  ground  motion  data  is  typically  available  either  only  as  ground 
accelerations,  or  as  a  triple  of  ground  accelerations,  velocities  and  displace-
ments.    Usually,  the  velocities  and  the  displacements  are  computed  from  the 
accelerations using specialized filtering and baseline correction techniques, e.g.  
see peer.berkeley.edu/smcat/process.html.  Either input is accepted, with each 
quantity  specified  as  a  load  curve.    Only  the  acceleration  and  the  velocity  is 
required in the latter case; LS-DYNA does not require the ground displacement.  
2. 
If only the ground acceleration data is provided for a particular ground motion, 
LS-DYNA generates a corresponding load curve for the velocity by integrating 
the acceleration numerically.  The generated load curves are printed out to the 
D3HSP file.  It is up to the user to ensure that these generated load curves are 
satisfactory for the analysis.
*DEFINE 
Purpose:    To  model  the  heat  affect  zone  in  a  welded  structure,    the  yield  stress  and 
failure strain are scaled in shell models as a function of their distance from spot welds 
and the nodes specified in *DEFINE_HAZ_TAILOR_WELDED_BLANK.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ID_HAZ 
IOP 
PID 
PID_TYP 
Type 
Default 
I 
0 
  Card 2 
1 
I 
0 
2 
I 
0 
3 
I 
0 
4 
Variable 
ISS 
IFS 
ISB 
IFB 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
5 
ISC 
I 
0 
6 
IFC 
I 
0 
7 
8 
ISW 
IFW 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
ID_HAZ 
Property set ID.  A unique ID number must be used. 
IOP 
Activity  flag.    If  IOP = 0,  then  the  scaling  is  not  applied,  and  if 
IOP = 1, the scaling is active. 
PID 
Part or part set ID. 
PID_TYP 
ISS 
PID  type.    PID_TYP = 0  indicates  that  PID  is  a  *PART  ID,  and 
PID_TYP = 1, a part set. 
Curve ID for scaling the yield stress based on the distance to the
closest  solid  element  spot  weld.    Use  a  negative  ID  for  curves
normalized  by  the  spot  weld  diameter  as  described  in  the
Remarks below.
*DEFINE_HAZ_PROPERTIES 
DESCRIPTION
IFS 
ISB 
IFB 
ISC 
IFC 
ISW 
IFW 
Curve ID for scaling the failure strain based on the distance to the
closest  solid  element  spot  weld.    Use  a  negative  ID  for  curves
normalized  by  the  spot  weld  diameter  as  described  in  the
Remarks below. 
Curve ID for scaling the yield stress based on the distance to the 
closest  beam  element  spot  weld.    Use  a  negative  ID  for  curves
normalized  by  the  spot  weld  diameter  as  described  in  the
Remarks below. 
Curve ID for scaling the failure strain based on the distance to the
closest  beam  element  spot  weld.    Use  a  negative  ID  for  curves 
normalized  by  the  spot  weld  diameter  as  described  in  the
Remarks below. 
Curve ID for scaling the yield stress based on the distance to the
closest    constrained  spot  weld.    Use  a  negative  ID  for  curves
normalized  by  the  spot  weld  diameter  as  described  in  the
Remarks below. 
Curve ID for scaling the failure strain based on the distance to the
closest  constrained  spot  weld.    Use  a  negative  ID  for  curves
normalized  by  the  spot  weld  diameter  as  described  in  the
Remarks below. 
Curve ID for scaling the yield stress based on the distance to the
closest  tailor  welded  blank  node.    Use  a  negative  ID  for  curves
normalized  by  the  spot  weld  diameter  as  described  in  the
Remarks below. 
Curve ID for scaling the failure strain based on the distance to the 
tailor  welded  blank  node.    Use  a  negative  ID  for  curves
normalized  by  the  spot  weld  diameter  as  described  in  the
Remarks below. 
Remarks: 
The  yield  stress  and  failure  strain  are  assumed  to  vary  radially  as  a  function  of  the 
distance of a point to its neighboring spot welds.  Since larger spot welds may have a 
larger  radius  of  influence,  the  smallest  scale  factor  for  the  yield  stress  from  all  the 
neighboring  spot  welds  is  chosen  to  scale  the  yield  stress  at  a  particular  point.    The 
failure strain uses the scaling curve for the same weld.
Curve IDs may be input as negative values to indicate that they are normalized by the 
diameter of the spot weld to compensate for the effects of the spot weld size.  When this 
option is used, the scale factor is  calculated  based on the  distance  divided by the spot 
weld diameter for the spot weld that is closest to the element. 
The distance from a spot weld (or node for the blank) is measured along the surface of 
the parts in the part set.  This prevents the heat softening effects of a weld from jumping 
across empty space. 
The  HAZ  capability  only  works  with  parts  with  materials  using  the  STOCHASTIC 
option.  It may optionally be simultaneously used with *DEFINE_STOCHASTIC_VARI-
ATION  to  also  account  for  the  spatial  variations  in  the  material  properties.    See  *DE-
FINE_STOCHASTIC_VARIATION for more details.
*DEFINE_HAZ_TAILOR_WELDED_BLANK 
Purpose:    Specify  nodes  of  a  line  weld  such  as  in  a  Tailor  Welded  Blank.    The  yield 
stress  and  failure  strain  of  the  shell  elements  in  the  heat  affected  zone  (HAZ)  of  this 
weld are scaled according to *DEFINE_HAZ_PROPERTIES. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IDTWB 
IDNS 
Type 
Default 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
IDTWB 
Tailor Welded Blank ID 
IDNS 
Node Set ID defining the location of the line weld.
*DEFINE_HEX_SPOTWELD_ASSEMBLY_{OPTION} 
Purpose:    Define  a  list  of  hexahedral  elements  that  make  up  a  single  spot  weld  for 
computing the force and moment resultants that are written into the swforc output file.  
A  maximum  of  16  elements  may  be  used  to  define  an  assembly  representing  a  single 
spot weld.  See Figure 15-45.  This table of element IDs is generated automatically when 
beam  elements  are  converted  to  solid  elements.    See  the  input  parameter  RPBHX 
associated with the keyword *CONTROL_SPOTWELD_BEAM. 
Available options for this command are:   
<BLANK> 
N 
For the <BLANK> option, all solid elements specified on Card 2 make up the spot weld 
and no additional card is read.  For the N option, N is an integer representing the total 
number  of  solid  elements  making  up  the  spot  weld.    If  N  is  greater  than  8,  the 
additional card beyond Card 2 is read.  N may not exceed 16. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ID_SW 
Type 
Default 
I 
0 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EID1 
EID2 
EID3 
EID4 
EID5 
EID6 
EID7 
EID8 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I
Figure  15-45.    Illustration  of  four,  eight,  and  sixteen  element  assemblies  of
solid hexahedron elements forming a single spot weld. 
Additional card for N > 8. 
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EID9 
EID10 
EID11 
EID12 
EID13 
EID14 
EID15 
EID16 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
ID_SW 
Spot weld ID.  A unique ID number must be used. 
EIDn 
Element ID n for up to 16 solid hexahedral elements. 
Remarks: 
The elements comprising a spot weld assembly may share a part ID (PID) with elements 
in  other  spot  weld  assemblies  defined  using  *DEFINE_HEX_SPOTWELD_ASSEMBLY 
but  may  not  share  a  PID  or  even  a  material  ID  (MID)  with  elements  that  are  not 
included in a *DEFINE_HEX_SPOTWELD_ASSEMBLY.
*DEFINE_LANCE_SEED_POINT_COORDINATES 
Purpose:  The keyword is to activate the trimming in lancing.  It is used in conjunction 
with  *ELEMENT_LANCING  to  define  a  seed  point  which  would  be  on  the remaining 
part after lancing and trim. 
  Card 1 
1 
Variable 
NSEED 
Type 
I 
Default 
none 
2 
X1 
F 
0 
3 
Y1 
F 
0 
4 
Z1 
F 
0 
5 
X2 
F 
0 
6 
Y2 
F 
7 
Z2 
F 
0.0 
0.0 
8 
  VARIABLE   
DESCRIPTION
NSEED 
Number of seed points.  Maximum value of “2” is allowed. 
X1, Y1, Z1 
Location coordinates of seed point #1. 
X2, Y2, Z2 
Location coordinates of seed point #2. 
Remarks: 
1.  This keyword will remove all scraps during or after lancing, dependent on how 
the  parameter  AT  is  defined  in  *ELEMENT_LANCING.    Lancing  curves  must 
form a closed loop, meaning first and last point coordinates must be coincident.  
Scraps are the portions that are exclusive of the portions whose seed points are 
defined by this keyword. 
2.  The following input defines two sets of seed point coordinates, where a double-
attached part may be lanced and trimmed: 
*DEFINE_LANCE_SEED_POINT_COORDINATES 
$    NSEED        X1       Y1         Z1       X2        Y2        Z2 
         2    -289.4    98.13   2354.679   -889.4    91.13    255.679 
3.  Refer to manual pages in *ELEMENT_LANCING for more details. 
Revision Information 
This feature is available in LS-DYNA Revision 107262 and later releases.
:
*DEFINE 
Purpose:    To  control  the  content  of  the  history  variables  in  the  d3plot  database.    This 
feature is supported for solid, beam and shell elements. 
Define as many cards as needed to define the extra history variables.  This input ends at 
the next keyword “*” card. 
  Card 1 
Variable 
Type 
Default 
1 
LABEL 
A40 
none 
2 
A1 
F 
3 
A2 
F 
4 
A3 
F 
5 
A4 
F 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
LABEL 
String identifying history variable type. 
An 
Attributes, see discussion below. 
Remarks: 
Material  models  in  LS-DYNA  use  history variables  that  are  specific  to the  constitutive 
model being used.  For most materials, 6 are reserved for the Cauchy stress components 
and 1 for the effective plastic strain, but many models have more than that.  The history 
variables  may  include  interesting  physical  quantities  like  material  damage,  material 
phase  compositions,  strain  energy  density  and  strain  rate,  but,  in  addition,  they  may 
also  include  nonphysical  quantities  like  material  direction  cosines,  scale  factors  and 
parameters that are used for the numerical algorithms but hard to interpret when post-
processed. 
By  using  NEIPS,  NEIPB  and  NEIPH  on  *DATABASE_EXTENT_BINARY,  these  extra 
history variables can be exported to the d3plot database in the order that they are stored, 
and  in  LS-PrePost  the  variables  may  then  be  plotted  (Hist  button)  or  fringed  (Misc 
menu).    There  are  a  few  drawbacks  with  this  approach.    The  user  must,  for  instance, 
have knowledge of the storage location of a certain history variable for a given material 
model  and  element  type.    While  this  information  can  be  retrieved  either  in  the  LS-
DYNA  manual,  on  LS-DYNA  support  sites  or  in  LS-PrePost  itself,  it  is  not  always 
convenient.
Furthermore,  the  same  physical  quantity  may  be  stored  in  different  locations  for 
different  materials  and  different  element  types,  meaning  that  history  variable  #1  will 
correspond  to  different  things  in  different  parts  which  complicate  post-processing  of 
large models.  The user may also be interested in a certain material specific quantity that 
is not necessarily stored as a history variable, this is not retrievable using this approach.  
Finally,  if  the  history  variable  of  interest  happens  to  be  stored  in  a  bad  location,  i.e., 
among  the  last  ones  in  a  long  list,  it  would  be  necessary  to  set  NEIPS,  NEIPB  and/or 
NEIPH  large  enough  to  access  this  variable  in  LS-PrePost.    This  could  result  in 
unnecessarily large binary plot files. 
The present keyword is an attempt to organize the extra history variables with respect 
to uniformity, a goal is to get an output that is reasonably small and easy to interpret.  
The  input  is  very  simple,  use  the  keyword  *DEFINE_MATERIAL_HISTORIES  in  the 
keyword  input  deck,  followed  by  lines  that  specify  the  history  variables  of  interest 
using  predetermined  labels  and  attributes.    NEIPS,  NEIPB  and  NEIPH  on  *DATA-
BASE_EXTENT_BINARY  will  then  be  overridden  by  the  number  of  history  variables, 
i.e., number of lines, requested on this card.  As an example 
*DEFINE_MATERIAL_HISTORIES 
Instability 
Damage 
would  mean  that  two  extra  history  variables  are  output  to  the  d3plot  database,  so 
NEIPS,  NEIPB  and  NEIPH  will  internally  be  set  to  2  regardless  of  the  user  input.  
History  variable  #1  will  correspond  to  an  instability  measure  (between  0  and  1)  and 
history  variable  #2  will  correspond  to  a  material  damage  (between  0  and  1),  i.e.,  the 
history variables are output in the order they are listed.  If there are several instances of 
this  keyword  in  an  input  deck,  then  the  order  of  the  history  variables  will  follow  the 
order that the cards are read by the keyword reader. 
In the d3hsp file the user may find the complete list by searching for the string “M a t e 
r i a l  H i s t o r y  L i s t”.  For a material that does not store or calculate an “instability” 
or  “damage”  history  variable, the  output  will  be  zero  and  thus  the  output  will  not  be 
cluttered by unwanted data.  Note that this keyword does not necessarily require that 
the history variable be stored, as long as it can be calculated when LS-DYNA outputs a 
plot state.  This opens for the possibility to request quantities that are not available by 
just using NEIPS, NEIPB and/or NEIPH on *DATABASE_EXTENT_BINARY.  
For  large  models  with  many  different  parts  and  materials,  the  Instability  or  Damage 
variables  should  provide  a  comprehensive  overview  and  understanding  of  the  critical 
areas in terms of failure that otherwise may not be assessable.  
The permitted LABELs (case-sensitive) are
Instability 
Damage 
A number between 0 and 1 that indicates how close a element 
or  integration  point  is  to  failure  or  to  initiate  damage,  no 
attributes apply to this label. 
A number between 0 and 1 indicating the damage level of the 
element or integration point, no attributes apply to this label. 
Plastic Strain Rate 
Effective  plastic  strain  rate,  calculated  generically  for  “all” 
plastic  materials  from  the  evolution  of  effective  plastic  strain, 
no attributes apply to this label. 
History 
Fetch  a  history  variable  at  a  known  place  for  a  given  material 
type, element type and part set.  The following attributes apply.
A1 
A2 
A3 
A4 
History variable location, mandatory. 
Material type, default applies to all materials. 
Element  type,  0  for  all  element  types,  1  for  solids,  2 
for shells and 3 for beams. 
Part  set,  history  will  only  be  fetched  from  the  parts 
in  the  given  part  set.    The  default  is  all  parts  in  the 
model. 
Examples: 
The History label is  for users who know where history variables of interest are stored 
and want to use this to compress or simplify the output.  An example is 
*DEFINE_MATERIAL_HISTORIES 
History,4,272,1,23 
History,1,81 
*SET_PART_LIST 
23 
2,3 
which  will make a list of two history variables in the output.  History variable #1 will 
fetch the 4th history variable, but displayed only for the RHT concrete model (material 
272), solid elements and in parts 2 and 3.   History variable #2 will fetch the 1st history 
variable, display it only for the plasticity with damage model (material 81), but for any 
element  and  part.    Both  of  these  requested  variables  happen  to  be  the  damage  in  the 
respective materials, so an alternative to do something similar would be to use 
*DEFINE_MATERIAL_HISTORIES 
Damage
for which the damage for all materials will be displayed in history variable #1. 
The  history  variables  that  may  be  requested  using  this  keyword  are  tabulated  in  the 
individual material model chapters, see Volume II of the Keyword Users’ Manual.  At 
the end of the remarks for a material model, a table such as the one below is present if 
there are retrievable history variables.   
*DEFINE_MATERIAL_HISTORIES Properties 
Label 
Attributes 
Description 
Instability 
Plastic Strain Rate 
- 
- 
- 
- 
- 
- 
- 
- 
𝑝 , see FAIL 
Failure indicator 𝜀eff
𝑝  
Effective plastic strain rate 𝜀̇eff
𝑝 /𝜀fail
Whether mentioned in such table or not, Plastic Strain Rate is available for any material 
model that calculates plastic strain as the 7th standard history variable.  Label in the table 
states  what  the  string  LABEL  on  *DEFINE_MATERIAL_HISTORIES  must  be,  a1  to  a4 
will  list  attributes  A1  to  A4  if  necessary,  and Description  will  be  a  short  description  of 
what is output with this option, including possible restrictions.  Further development of 
this  keyword  will  mainly  be  driven  by  customer  requests  submitted  to  sugges-
tions@lstc.com.    Currently  only  solid,  beam  and  shell  elements  are  supported  for  the 
binary d3plot format, a goal is to include thick shells and support ascii/binout output in 
future versions of LS-DYNA. 
Note: 
The Labels are case-sensitive.
*DEFINE_MULTI_DRAWBEADS_IGES 
Purpose:    This  keyword  is  developed  to  simplify  the  creation  and  definition  of  draw 
beads, which previously required the use of many keywords. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME 
A80 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DBID 
VID 
PID 
BLKID 
NCUR 
Type 
I 
I 
Default 
none 
none 
I 
1 
I 
1 
I 
none 
IGES  Curve  ID  cards.    For  multiple  draw  bead  curves  include  as  many  cards  as 
necessary.  Input is terminated at the next (“*”) card. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CRVID 
BFORCE 
Type 
I 
F 
Default 
none 
0.0 
  VARIABLE   
DESCRIPTION
DBID 
VID 
Draw  bead  set  ID,  which  may  consists  many  draw  bead
segments. 
Vector ID, as defined by *DEFINE_VECTOR.  This vector is used 
to  project  the  supplied  curves  to  the  rigid  tool,  defined  by  the
parameter PID below.
Part  ID  of  a  rigid  tool  to  which  the  curves  are  projected  and
attached. 
Part ID of the blank. 
Number of draw bead curve segments (in the IGES file defined by 
FILENAME) to be defined. 
IGES curve ID for each segment. 
Draw bead force for each segment. 
*DEFINE 
  VARIABLE   
PID 
BLKID 
NCUR 
CVRID 
BFORCE 
Remarks: 
1.  This keyword alone can be used to define draw bead forces around a stamping 
part.    The  following  partial  keyword  example  shows  a  draw  bead  set  with  ID 
98,  consists  of  three  curves  with  ID,  12,  23,  and  45,  each  with  bead  forces  of 
102.1,  203.3,  142.5  Newton/mm,  respectively,  are  being  created  for  blank  with 
part  ID  1.    The  beads  are  projected  along  vector  ID  99,  and  are  attached  to  a 
rigid tool with part ID 3.  The IGES file to define the draw bead curve is “draw-
beads3.iges”. 
*DEFINE_MULTI_DRAWBEADS_IGES 
drawbead3.iges 
$     DBID       VID       PID     BLKID      NCUR 
        98        99         3         1         3 
$    CRVID    BFORCE 
        12     102.1 
        23     203.3 
        45     142.5 
*define_vector 
99,0.0,0.0,0.0,0.0,0.0,1.0 
Revision information: 
This feature is available in LS-DYNA R5 Revision 62840 and later releases.
*DEFINE 
Purpose:  To define a simple geometry for initial air domain. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
GID 
GTYPE1 
GTYPE2 
Type 
Default 
  Card 2 
Variable 
I 
0 
1 
XA 
Type 
F 
Default 
0. 
  Card 3 
Variable 
1 
X0 
Type 
F 
Default 
0. 
  Card 4 
Variable 
1 
XC 
Type 
F 
Default 
0. 
I 
0 
2 
YA 
F 
0. 
2 
Y0 
F 
0. 
2 
YC 
F 
0. 
I 
0 
3 
ZA 
F 
0. 
3 
Z0 
F 
0. 
3 
ZC 
F 
0. 
7 
8 
7 
8 
7 
8 
4 
XB 
F 
0. 
4 
G1 
F 
0. 
4 
G4 
F 
0. 
5 
YB 
F 
0. 
5 
G2 
F 
0. 
5 
G5 
F 
0. 
6 
ZB 
F 
0. 
6 
G3 
F 
0. 
6 
G6 
F 
0.
VARIABLE   
DESCRIPTION
GID 
ID of a GEOMETRY defining initial air particle domain. 
GTYPE1 
GTYPE2 
Geometry type 
EQ.1:  box 
EQ.2:  sphere 
EQ.3:  cylinder 
EQ.4:  ellipsoid 
EQ.5:  hemisphere  
XA, YA, ZA 
(XA, YA, ZA) defines a vector of the 𝑥-axis 
XB, YB, ZB 
(XB, YB, ZB) defines a vector of the 𝑦-axis 
X0, Y0, Z0 
Center coordinates of air domain 
G1 
Dimension value depending on GTYPE. 
GTYPE.EQ.1: length of 𝑥 edge 
GTYPE.EQ.2: Radius of sphere 
GTYPE.EQ.3: Radius of cross section 
GTYPE.EQ.4: length of 𝑥-axes   
GTYPE.EQ.5: Radius of hemisphere 
G2 
Dimension value depending on GTYPE. 
GTYPE.EQ.1:  length of 𝑦 edge 
GTYPE.EQ.3:  length of cylinder  
GTYPE.EQ.4:  length of 𝑦-axes   
G3 
Dimension value depending on GTYPE. 
GTYPE.EQ.1: length of 𝑧 edge 
GTYPE.EQ.4: length of 𝑧-axes 
XC, YC, ZC 
Center coordinates of domain excluded from the air domain 
G4, G5, G6 
See definition of G1, G2, G3
*DEFINE 
1. 
If  GTYPE1/GTYPE2  is  5,  the  hemisphere  is  defined  in  negative  𝑧  direction 
defined by the cross product of the 𝑦 and 𝑥 axis.
*DEFINE_PBLAST_GEOMETRY 
Purpose:  To define a simple geometry for high explosives domain. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
GID 
GTYPE 
Type 
Default 
  Card 2 
Variable 
I 
0 
1 
XA 
Type 
F 
Default 
0. 
  Card 3 
Variable 
1 
Xc 
Type 
F 
Default 
0. 
  Card 4 
Variable 
1 
G1 
Type 
F 
Default 
0. 
15-212 (DEFINE) 
I 
0 
2 
YA 
F 
0. 
2 
Yc 
F 
0. 
2 
G2 
F 
0. 
3 
ZA 
F 
0. 
3 
Zc 
F 
0. 
3 
G3 
F 
0. 
7 
8 
4 
XB 
F 
0. 
5 
YB 
F 
0. 
6 
ZB 
F 
0. 
4 
5 
6 
7 
8 
4 
5 
6
VARIABLE   
DESCRIPTION
GID 
ID of a GEOMETRY defining high explosive particle domain. 
GTYPE 
Geometry type 
EQ.1:  box 
EQ.2:  sphere 
EQ.3:  cylinder 
EQ.4:  ellipsoid 
EQ.5:  hemisphere  
XA, YA, ZA 
(XA, YA, ZA) defines a vector of the x-axis 
XB, YB, ZB 
(XB, YB, ZB) defines a vector of the y-axis 
XC 
YC 
ZC 
G1 
G2 
G3 
X-coordinate of charge center 
Y-coordinate of charge center 
Z-coordinate of charge center 
GTYPE.EQ.1:  length of X edge 
GTYPE.EQ.2:  Radius of sphere 
GTYPE.EQ.3:  Radius of cross section 
GTYPE.EQ.4:  length of X-axes   
GTYPE.EQ.5:  Radius of hemisphere 
GTYPE.EQ.1:  length of Y edge 
GTYPE.EQ.3:  length of cylinder  
GTYPE.EQ.4:  length of Y-axes   
GTYPE.EQ.1:  length of Z edge 
GTYPE.EQ.4:  length of Z-axes 
Remarks: 
1. 
If GTYPE is 5, the hemisphere is defined in negative Z direction defined by the 
cross product of the Y and X axis.
*DEFINE_PLANE 
Purpose:    Define  a  plane  with  three  non-collinear  points.    The  plane  can  be  used  to 
define a reflection boundary condition for problems like acoustics. 
  Card 1 
1 
Variable 
PID 
Type 
Default 
  Card 2 
Variable 
I 
0 
1 
X3 
Type 
F 
2 
X1 
F 
3 
Y1 
F 
4 
Z1 
F 
5 
X2 
F 
6 
Y2 
F 
7 
Z2 
F 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
4 
5 
6 
7 
2 
Y3 
F 
3 
Z3 
F 
8 
CID 
I 
0 
8 
Default 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
PID 
Plane ID.  A unique number has to be defined. 
X1 
Y1 
Z1 
X2 
Y2 
Z2 
CID 
X-coordinate of point 1. 
Y-coordinate of point 1. 
Z-coordinate of point 1. 
X-coordinate of point 2. 
Y-coordinate of point 2. 
Z-coordinate of point 2. 
Coordinate  system  ID  applied  to  the  coordinates  used  to  define
the current plane.  The coordinates X1, Y1, Z1, X2, Y2, Z2, X3, Y3
and Z3 are defined with respect to the coordinate system CID. 
X3 
X-coordinate of point 3.
VARIABLE   
DESCRIPTION
Y3 
Z3 
Y-coordinate of point 3. 
Z-coordinate of point 3. 
Remarks: 
1.  The  coordinates  of  the  points  must  be  separated  by  a  reasonable  distance  and 
not collinear to avoid numerical inaccuracies.
Available options include: 
ALE 
LAGRANGIAN 
*DEFINE_POROUS 
Purpose:    The  *DEFINE_POROUS_ALE  card  defines  the  Ergun  porous  coefficients  for 
ALE elements.  It is to be used with *LOAD_BODY_POROUS.  This card with the LA-
GRANGIAN  option, 
the  porous 
coefficients  for  Lagrangian  elements  and  is  to  be  used  with  *CONSTRAINED_LA-
GRANGE_IN_SOLID (slave parts with CTYPE = 11 or 12). 
*DEFINE_POROUS_LAGRANGIAN,  defines 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EIDBEG 
EIDEND 
LOCAL 
VECID1 
VECID2  USERDEF 
Type 
I 
Default 
none 
  Card 2 
1 
I 
0 
2 
I 
0 
3 
I 
0 
4 
I 
0 
5 
I 
0 
6 
Variable 
Axx 
Axy 
Axz 
Bxx 
Bxy 
Bxz 
Type 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
7 
8 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Ayx 
Ayy 
Ayz 
Byx 
Byy 
Byz 
Type 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0
Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Azx 
Azy 
Azz 
Bzx 
Bzy 
Bzz 
Type 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
EIDBEG, 
EIDEND 
DESCRIPTION
EIDBEG, EIDEND > 0: 
EIDBEG, EIDEND < 0: 
Range  of  thick  porous  element  IDs. 
These  are  solids  in  3D  and  shells  in 
2D. 
Range  of  thin  porous  element  IDs. 
These are shells in 3D and beams in 
2D.    The  ALE  option  does  not  sup-
port thin porous elements. 
EIDBEG > 0, EIDEND = 0:  EIDBEG  is  a  set  of  thick  porous 
elements 
EIDBEG > 0, EIDEND < 0:  EIDBEG  is  a  set  of  thin  porous 
elements 
LOCAL 
Flag to activate an element coordinate system: 
EQ.0: The forces are applied in the global directions. 
EQ.1: The  forces  are  applied  in  a  local  system  attached  to  the
element.    The  system  is  consistent  with  DIREC = 1  and 
CTYPE = 12 in *CONSTRAINED_LAGRANGE_IN_SOL-
ID.  For CTYPE = 11, LOCAL is always 1 and the 𝑥-axis is 
aligned with the element normal while the 𝑦-axis passes 
through the element center and the first node in the ele-
ment  connectivity  (*ELEMENT_BEAM  in  2D  or  *ELE-
MENT_SHELL in 3D)
VECID1, 
VECID2 
*DEFINE_POROUS 
DESCRIPTION
*DEFINE_VECTOR  IDs  to  define  a  specific  coordinate  system.
VECID1  and  VECID2  give  the  𝑥-  and  𝑦-direction  respectively. 
The  𝑧-vector  is  a  cross  product  of  VECID1  and  VECID2.    If  this
latter is not orthogonal to VECID1, its direction will be corrected
with a cross-product of 𝑧- and 𝑥-vectors.  The vectors are stored as 
isoparametric  locations  to  update  their  directions  if  the  element
deforms or rotates. 
USERDEF 
Flag to compute Aij and Bij with a user defined routine in the file 
dyn21.F  called  lagpor_getab_userdef.    The  file  is  part  of  the 
general package usermat. 
Viscous matrix for the porous flow Ergun equation.  : 
Inertial matrix for the porous flow Ergun equation.  : 
Aij 
Bij 
Remarks: 
1.  Ergun  Equation.    The  Ergun  equation  computing  the  pressure  gradient  along 
each direction 𝑖 = 𝑥, 𝑦, 𝑧 can be written as follows: 
𝑑𝑃
𝑑𝑥𝑖
= ∑[𝜇𝐴𝑖𝑗𝑉𝑗 + 𝜌𝐵𝑖𝑗∣𝑉𝑗∣𝑉𝑗]
𝑗=1
Where, 
a)  𝑉𝑖 is the relative velocity of the flow  in the porous media  
b)  𝐴𝑖𝑗 are the viscous coefficients of the Ergun-type porous flow equation in 
the ith direction..  This matrix is similar to the viscous coefficients used in 
*LOAD_BODY_POROUS. 
c)  𝐵𝑖𝑗   are  the  inertial  coefficient  of  the  Ergun-type  porous  flow  equation  in 
the  ith  direction.    This  matrix  is  similar  to  the  inertial  coefficients  used  in 
*LOAD_BODY_POROUS. 
If  this  keyword  defines  the  porous  properties  of  Lagrangian  elements  in 
*CONSTRAINED_LAGRANGE_IN_SOLID,  the  porous  coupling  forces  are 
computed  with  the  pressure  gradient  as  defined  above  instead  of  the  equa-
tions used for CTYPE = 11 and 12.
*DEFINE 
Purpose:  Defines a closed gas filled tube for the simulation of interior pressure waves 
that result from changes in the tube cross section area over time.  The tube is defined by 
tubular  beam  elements,  and  the  gas  volume  is  determined  by  beam  cross  section  area 
and  initial  element  lengths.    Area  changes  are  given  by  contact  penetration  from 
surrounding  elements  (only  mortar  contacts  currently  supported).    The  pressure 
calculation is not coupled with the deformation of the beam elements and does not use 
any data from the material card.  Pressure and tube area at the beam nodes are output 
through *DATABASE_PRTUBE. 
4 
5 
6 
7 
8 
  Card 1 
1 
Variable 
PID 
Type 
Default 
I 
0 
Optional card 
2 
WS 
F 
3 
PR 
F 
0.0 
0.0 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VISC 
CFL 
DAMP 
Type 
F 
F 
F 
Default 
1.0 
0.9 
0.0
PID 
*DEFINE_PRESSURE_TUBE 
DESCRIPTION
Part  ID  of  tube.  All  connected  beam  elements  in  the  part  will 
model  a    closed  tube.    Only  tubular  beam  elements  are  allowed, 
i.e.    ELFORM = 1,4,5,11  with  CST = 1  on  *SECTION_BEAM.
Initial  tube  cross  section  area  is  calculated  using  the  beam  inner
diameter  TT1/TT2.    If  no  inner  diameter  is  given,  the  outer
diameter TS1/TS2 is used. 
The  beam  elements  may  not  contain  junctions  and  two  different 
parts  where  *DEFINE_PRESSURE_TUBE  is  applied  may  not 
share nodes.  For MPP all elements in the part will be on a single
processor. 
WS 
PR 
VISC 
CFL 
Speed of sound 𝑐0 in the gas 
Initial gas pressure 𝑝0 inside tube 
Artificial viscosity multiplier 𝒗, see remarks 
CFL-factor 𝒌, see remarks 
DAMP 
Linear damping 𝒅, see remarks 
Remarks:  
The  pressure  tube  is  modeled  with  an  acoustic  approximation  of  the  1D  compressible 
Euler equations for pipes with varying thickness 
𝜕
𝜕𝑡
(𝜌𝐴) +
𝜕
𝜕𝑥
(𝜌𝑢𝐴) = 0, 
𝜕
𝜕𝑡
(𝜌𝑢𝐴) +
𝜕
𝜕𝑡
(𝐸𝐴) +
𝜕
𝜕𝑥
𝜕
𝜕𝑥
(𝜌𝑢2𝐴 + 𝑝𝐴) = 𝑝
𝜕𝐴
𝜕𝑥
, 
(𝑢(𝐸 + 𝑝)𝐴) = 0, 
where  𝐴 = 𝐴(𝑥, 𝑡)  is  the  cross  section  area  and  𝜌, 𝑝, 𝑢, 𝐸  is  density,  pressure,  velocity, 
and  energy  per  unit  volume,  respectively.    The  above  system  is  closed  under  the 
constitutive relations 
𝐸 = 𝜌𝑒 +
𝜌𝑢2
,
𝑝 = 𝑝(𝜌, 𝑒), 
where 𝑒 is the internal energy per unit mass.  
For an isentropic and isothermal flow, the pressure will be proportional to the density, 
i.e. 
𝑝 = 𝑐0
2𝜌,
and  the  energy  equation  can  be  dropped.    This  is  a  good  approximation  of  the  Euler 
equations for acoustic flows where the state variables are smooth perturbations around 
a  background  state.    For  such  flows  no  shocks  will  develop  over  time  but  may  be 
present from initial/boundary values or source terms.  
Assuming  small  perturbations,  linearization  around  (𝜌0, 𝑝0, 𝑢0 = 0)  gives  the  acoustic 
approximation 
𝜕𝑦
𝜕𝑥
𝜕
𝜕𝑡
𝜕𝑦
𝜕𝑡
(𝐴𝜌) + 𝜌0
2 𝜕
𝜕𝑥
+ 𝑐0
𝜌0
(𝐴𝜌) = 𝑝
= 0, 
𝜕𝐴
, 
𝜕𝑥
where 𝑦 = 𝐴𝑢.  Expressed in 𝑦 and 𝑝 we have 
𝜕𝑝
𝜕𝑡
+
𝜕 ln 𝐴
𝜕𝑡
𝜕𝑦
𝜕𝑡
𝑝 +
+ 𝐴
𝑝0
𝑐0
𝑝0
𝜕𝑦
𝜕𝑥
𝜕𝑝
𝜕𝑥
= 0, 
= 0. 
This  linearized  system  is  solved  using  the  standard  Galerkin  finite  element  method, 
using piecewise linear basis functions and artificial viscosity.  Linear damping is added 
to model energy losses from friction between the gas and the tube walls.  With artificial 
viscosity and linear damping, the system can be written as 
𝜕𝑝
𝜕𝑡
+
𝜕 ln 𝐴
𝜕𝑡
𝜕𝑦
𝜕𝑡
𝑝 +
+ 𝐴
𝑝0
𝑐0
𝑝0
𝜕𝑦
𝜕𝑥
𝜕𝑝
𝜕𝑥
= 𝜖
= 𝜖
𝜕2𝑝
𝜕𝑥2 − 𝒅(𝑝 − 𝑝0) 
𝜕2𝑦
𝜕𝑥2, 
where  the  artificial  viscosity  is  proportional  to  the  maximum  initial  beam  element 
length, i.e. 
𝜖 = 𝒗𝑐0 max
Δ𝑥𝑖, 
Time integration is independent of the mechanical solver and uses a step size less than 
or equal to the global time step, satisfying a CFL condition 
Δ𝑡 < min
𝒌Δ𝑥𝑖
Δ𝑥𝑖 ∣𝜕 ln 𝐴
𝜕𝑡
∣ + 3𝑐0
.
*DEFINE_REGION 
Purpose:  Define a volume of space, optionally in a local coordinate system. 
  Card 1 
Variable 
1 
ID 
Type 
I 
2 
3 
4 
5 
6 
7 
8 
TITLE 
A70 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TYPE 
CID 
Type 
I 
I 
Card 3 for Rectangular Prism.  Use when type = 0. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
XMN 
XMX 
YMN 
YMX 
ZMN 
ZMX 
Type 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Card 3 for Sphere.  Use when type = 1. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
XC1 
YC1 
ZC1 
RMIN1 
RMAX1 
Type 
R 
R 
R 
R 
R 
Default 
0.0 
0.0 
0.0 
0.0 
0.0
Card 3 for Cylinder.  Use when type = 2. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
XC2 
YC2 
ZC2 
AX2 
AY2 
AZ2 
RMIN2 
RMAX2 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Card 4 for Cylinder.  Use when type = 2. 
2 
3 
4 
5 
6 
7 
8 
  Card 4 
Variable 
1 
L2 
Type 
F 
Default 
0.0 
Card 3 for Ellipsoid.  Use when type = 3. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
XC3 
YC3 
ZC3 
AX3 
AY3 
AZ3 
BX3 
BY3 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0
Card 4 for Ellipsoid.  Use when type = 3. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BZ3 
RA3 
RB3 
RC3 
Type 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
ID 
TITLE 
TYPE 
CID 
XMN 
YMN 
ZMN 
XMX 
YMX 
ZMX 
Region ID 
Title for this region 
Region type: 
EQ.0:  Box 
EQ.1:  Sphere or spherical shell 
EQ.2:  Cylinder or cylindrical shell, infinite or finite in length
EQ.3:  Ellipsoid 
Optional local coordinate system ID.  If given, all the following
input parameters will be interpreted in this coordinate system.
Lower 𝑥 limit of box 
Lower 𝑦 limit of box 
Lower 𝑧 limit of box 
Upper 𝑥 limit of box 
Upper 𝑦 limit of box 
Upper 𝑧 limit of box 
XC1, YC1, ZC1 
Coordinates of the center of the sphere 
RMIN1, RMAX1 
The inner and outer radii of the spherical shell.  Set RMIN1 = 0 
for a solid sphere 
XC2, YC2, ZC2 
A point on the cylindrical axis
VARIABLE   
DESCRIPTION
AX2, AY2, AZ2 
A vector which defines the direction of the axis of the cylinder
RMIN2, RMAX2 
The  inner  and  outer  radii  of  the  cylindrical  shell.    Set
RMIN2 = 0 for a solid cylinder 
L2 
Length  of  the  cylinder.    If  L2 = 0,  and  infinite  cylinder  is 
defined.    Otherwise  the  cylinder  has  one  end  at  the  point 
(XC2, YC2, ZC2) and the other at a distance L2 along the axis 
in the direction of the vector (AX2, AY2, AZ2) 
XC3, YC3, ZC3 
Coordinates of the center of the ellipsoid 
AX3, AY3, AZ3 
A vector in the direction of the first axis of the ellipsoid (axis 𝐚)
BX3, BY3, BZ3 
A  vector,  𝐛̃ ,  in  the  plain  of  the  first  and  second  axes  of  the
ellipsoid.  The third axis of the ellipsoid (axis 𝐜) will be in the 
direction of 𝐚 × 𝐛̃ and finally the second axis 𝐛 = 𝐜 × 𝐚 
RA3, RB3, RC3 
The semi-axis lengths of the ellipsoid
*DEFINE_SD_ORIENTATION 
Purpose:    Define  orientation  vectors  for  discrete  springs  and  dampers.    These 
orientation  vectors  are  optional  for  this  element  class.    Four  alternative  options  are 
possible.  With the first two options, IOP = 0 or 1, the vector is defined by coordinates 
and is fixed permanently in space.  The third and fourth option orients the vector based 
on the motion of two nodes, so that the direction can change as the line defined by the 
nodes rotates. 
Card 
1 
Variable 
VID 
Type 
Default 
I 
0 
Remarks 
none 
2 
IOP 
I 
0 
1 
3 
XT 
F 
4 
YT 
F 
5 
ZT 
F 
0.0 
0.0 
0.0 
6 
7 
8 
NID1 
NID2 
I 
0 
I 
0 
IOP = 0,1 IOP = 0,1 IOP = 0,1 IOP = 2,3 
IOP = 2,3 
  VARIABLE   
DESCRIPTION
VID 
IOP 
Orientation vector ID.  A unique ID number must be used. 
Option: 
EQ.0: deflections/rotations are measured and forces/moments 
applied along the following orientation vector. 
EQ.1: deflections/rotations are measured and forces/moments
applied  along  the  axis  between  the  two  spring/damper
nodes  projected  onto  the  plane  normal  to  the  following
orientation vector. 
EQ.2: deflections/rotations are measured and forces/moments
applied  along  a  vector  defined  by  the  following  two
nodes. 
EQ.3: deflections/rotations are measured and forces/moments
applied  along  the  axis  between  the  two  spring/damper
nodes  projected  onto  the  plane  normal  to  the  a  vector 
defined by the following two nodes. 
XT 
YT 
x-value of orientation vector.  Define if IOP = 0,1. 
y-value of orientation vector.  Define if IOP = 0,1.
VARIABLE   
DESCRIPTION
z-value of orientation vector.  Define if IOP = 0,1. 
Node 1 ID.  Define if IOP = 2,3. 
Node 2 ID.  Define if IOP = 2, 3. 
ZT 
NID1 
NID2 
Remarks: 
1.  The  orientation  vectors  defined  by  options  0  and  1  are  fixed  in  space  for  the 
duration  of  the  simulation.    Options  2  and  3  allow  the  orientation  vector  to 
change with the motion of the nodes.  Generally, the nodes should be members 
of  rigid  bodies,  but  this  is  not  mandatory.    When  using  nodes  of  deformable 
parts  to  define  the  orientation  vector,  care  must  be  taken  to  ensure  that  these 
nodes will not move past each other.  If this happens, the direction of the orien-
tation vector will immediately change with the result that initiate severe insta-
bilities can develop.
*DEFINE_SET_ADAPTIVE 
Purpose:  To control the adaptive refinement level by element or part set. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SETID 
STYPE 
ADPLVL 
ADPSIZE 
Type 
I 
I 
I 
F 
Default 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
SETID 
STYPE 
Element set ID or part set ID 
Set type for SETID:   1-element set   2-part set 
ADPLVL 
Adaptive refinement level for all elements in SETID set. 
ADSIZE 
Minimum  element  size  to  be  adapted  based  on  element  edge 
length for all elements in SETID set. 
Remarks: 
1.  This option is for 3D-shell h-adaptivity only at the present time. 
2.  The order of defining refinement level for any elements is *CONTROL_ADAP-
TIVE and *DEFINE_BOX_ADAPTIVE. 
3. 
If  there  are  multiple  definitions  of  refinement  level  or  element  size  for  any 
elements, the latter one will be used.
*DEFINE 
Purpose:  The purpose of this keyword is to increase the efficiency of the SPH method’s 
neighborhood search algorithm by specifying an active region.  All SPH elements located 
outside  of  the  active  region  are  deactivated.    This  card  supports  active  regions 
consisting  of  the  volume  bounded  by  two  closed  surfaces  (boxes,  centered  cylinders, 
and centered spheres are currently supported).  Once the SPH particle is deactivated, it 
will stay inactive. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
TYPE 
STYPE 
CYCLE 
Type 
I 
Default 
none 
I 
0 
I 
0 
I 
1 
  VARIABLE   
DESCRIPTION
ID 
TYPE 
Part Set ID/Part ID 
EQ.0: Part set 
EQ.1: Part 
STYPE 
Type of the region. 
EQ.0: Rectangular box 
EQ.1: Cylinder 
EQ.2: Sphere 
CYCLE 
Number of cycles between each check
Interior Rectangular Box Card.  Card 2 format used for STYLE = 0. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
XIMIN 
YIMIN 
ZIMIN 
XIMAX 
YIMAX 
ZIMAX 
Type 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
Outer Rectangular Box Card.  Card 3 format used for STYPE = 0. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
XOMIN 
XOMIN 
ZOMIN 
XOMAX 
YOMAX 
ZOMAX 
Type 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
VARIABLE 
XIMIN, YIMIN, 
ZIMIN 
XIMAX, YIMAX, 
ZIMAX 
XOMIN, YOMIN, 
ZOMIN 
XOMAX, YOMAX, 
ZOMAX 
DESCRIPTION
Minimum x, y, z coordinate of the inner box 
Maximum x, y, z coordinates of the inner box 
Minimum x, y, z coordinate of the outer box 
Maximum x, y, z coordinates of the outer box
Cylinder Axis Card.  Card 2 format used for STYPE = 1.   
  Card 2 
Variable 
1 
X0 
Type 
F 
2 
Y0 
F 
3 
Z0 
F 
4 
XH 
F 
5 
YH 
F 
6 
ZH 
F 
7 
8 
Default 
none 
none 
none 
none 
none 
none 
Cylinder Radii Card.  Card 3 format used for STYPE = 1. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RMIN 
ZMIN 
RMAX 
ZMAX 
Type 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
VARIABLE 
X0, Y0, Z0 
DESCRIPTION
Coordinates  of  the  center  of  the  cylinder  base.    The  nested
cylinders  are  sharing  the  same  starting  base  plane.    This
point  also  serves  as  the  tail  for  the  vector  specifying  the
direction of the cylinders’ axis.   
XH, YH, ZH 
Coordinates  for  the  head  of  the  cylinders  axial  direction 
vector. 
RMIN, ZMIN 
Radius and length of the interior cylinder. 
RMAX, ZMAX 
Radius and length of the outer cylinder.
Center of Sphere Card.  Card 2 used for STYPE = 2. 
4 
5 
6 
7 
8 
  Card 2 
Variable 
1 
X0 
Type 
F 
2 
Y0 
F 
3 
Z0 
F 
Default 
none 
none 
none 
Sphere Radii Card.  Card 3 used for STYPE = 2. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RMIN 
RMAX 
Type 
F 
F 
Default 
none 
none 
VARIABLE 
DESCRIPTION
X0, Y0, Z0 
The spheres’ center. 
RMIN 
RMAX 
Radius of the interior sphere 
Radius of the outer sphere 
Remarks: 
1.Cylindrical system for SPH active region
Figure 15-46.  Example DEFINE_SPH_ACTIVE_REGION
*DEFINE_SPH_DE_COUPLING_{OPTION} 
Purpose: Define a penalty based contact.  This option is to be used for the node to node 
contacts to couple SPH solver and discrete element sphere (DES) solver. 
The available options include: 
<BLANK> 
ID 
ID Card.  Additional card for ID keyword option.  
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DID 
Type 
I 
Default 
none 
HEADING 
A80 
none 
SPH Part Cards.  Provide as many as necessary.  Input ends at the next keyword (“*”) 
card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SPHID 
DESID 
SPHTYP 
DESTYP 
PFACT 
DFACT 
SPHBOX 
Type 
I 
I 
I 
I 
F 
F 
I 
Default 
none 
none 
none 
none 
1.0 
0. 
none 
  VARIABLE   
DESCRIPTION
DID 
Definition ID.  This must be a unique number. 
HEADING 
Definition descriptor.  It is suggested that unique descriptions be
used. 
SPHID 
DESID 
SPH part or part set ID. 
DES part or part set ID.
SPHTYP 
SPH part type: 
EQ.0: Part set ID, 
EQ.1: Part ID. 
DESTYP 
DES part type: 
EQ.0: Part set ID, 
EQ.1: Part ID. 
PFACT 
Penalty scale factor 
DFACT 
Penalty scale factor for contact damping coefficient 
SPHBOX 
BOX ID for SPH parts, See Remark 1. 
Remarks: 
SPHBOX is used to define the box IDs for the SPH parts.  Only the particles that inside 
the boxes are defined for the node to node contacts.
*DEFINE_SPH_INJECTION 
Purpose:  This keyword injects SPH elements from user defined grid points. 
  Card 1 
1 
2 
3 
Variable 
PID 
NSID 
CID 
Type 
I 
I 
I 
4 
VX 
F 
5 
VY 
F 
6 
VZ 
F 
7 
8 
AREA 
F 
Default 
none 
none 
None 
0.0 
0.0 
0.0 
0.0 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TBEG 
TEND 
Type 
F 
F 
Default 
0.0 
1.0E20 
  VARIABLE   
DESCRIPTION
PID 
NSID 
CID 
Part ID of newly generated SPH elements. 
Node set ID.  Nodes are used for initial injection position for the
SPH elements. 
Local  coordinate  system  ID,  see  *DEFINE_COORDINATE_SYS-
TEM.    X  and  Y  coordinates  define  the  injection  plane,  Z
coordinate defines the normal to the injection plane. 
VX, VY, VZ 
Velocity of the inject elements: 𝐯 = (VX, VY, VZ) 
AREA 
TBEG 
TEND 
The area of initial injection surface.  The density of injection flow
comes from the material models see *MAT definition. 
Birth time 
Death time
*DEFINE_SPH_TO_SPH_COUPLING_{OPTION} 
Purpose: Define a penalty based contact.  This option is to be used for the node to node 
contacts between SPH parts. 
The available options include: 
<BLANK> 
ID 
ID Cards.  Additional card for ID keyword option. 
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DID 
Type 
I 
Default 
none 
Sets of coupling cards: 
HEADING 
A70 
none 
Each  set  consists  of  a  Card 1  and  may  include  an  additional  Card 2.    Unless  the  card 
following  Card 1  contains  an  “&”  in  its  first  column,  the  optional  card  is  not  read.  
Provide  as  many  sets  as  necessary.    This  input  terminates  at  the  next  keyword  (“*”) 
card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
MSID 
SSTYP 
MSTYP 
IBOX1 
IBOX2 
PFACT 
SRAD 
Type 
I 
I 
I 
I 
I 
I 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
1.0 
1.0
Optional.  The keyword reader identifies this card by an “&” in the first column. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DFACT 
ISOFT 
Type 
F 
Default 
0.0 
I 
0 
  VARIABLE   
DESCRIPTION
DID 
Definition ID.  This must be a unique number. 
HEADING 
Definition descriptor.  It is suggested that unique descriptions be
used. 
SSID 
MSID 
Slave part or part set ID. 
Master part or part set ID. 
SSTYP 
Slave part type: 
EQ.0: Part set ID, 
EQ.1: Part ID. 
MSTYP 
Master part type: 
EQ.0: Part set ID, 
EQ.1: Part ID. 
IBOX1 
IBOX2 
Box ID for slave parts, See Remark 1. 
Box ID for master parts, See Remark 1. 
PFACT 
Penalty scale factor, See Remark 2. 
SRAD 
Scale factor for nodes to nodes contact criteria, See Remark 3. 
DFACT 
Penalty scale factor for contact damping coefficient, See Remark 4.
Soft constraint option: 
     EQ.  0: penalty formulation 
     EQ.  1: soft constraint formulation 
The  soft  constraint  may  be  necessary  if  the  material  constants  of
the  parts  in  contact  have  a  wide  variation  in  the  elastic  bulk
moduli.    In  the  soft  constraint  option,  the  interface  stiffness  is
based on the nodal mass and the global time step size. 
ISOFT 
Remarks: 
1. 
IBOX1  and  IBOX2  are  used  to  define  the  box  IDs  for  the  slave  parts  and  the 
master parts respectively.  Only the particles that inside the  boxes are defined 
for the node to node contacts. 
2.  For High Velocity Impact problems, a smaller value (ranges from 0.01 to 1.0e-4) 
of PFACT variable is recommended.  A number ranges from 0.1 to 1 is recom-
mended for low velocity contact between two SPH parts. 
3.  Contact  between  two  SPH  particles  from  different  parts  is  detected  when  the 
distance  of  two  SPH  particles  is  less  than  SRAD*(sum  of  smooth  lengths  from 
two particles)/2.0. 
4.  DFACT = 0.0 is the default and is recommended.  For DFACT > 0.0, interaction 
between SPH parts includes a viscous effect, providing some stickiness similar 
to the particle approximation invoked when CONT = 0 in *CONTROL_SPH.  At 
present, no recommendation can be given for a value of DFACT other than the 
value should be less than 1.0. 
.
*DEFINE_SPOTWELD_FAILURE_{OPTION} 
The available options are 
<BLANK> 
ADD 
Purpose:    Define  spot  weld  failure  data  for  the  failure  criterion  developed  by  Lee  and 
Balur  (2011).    This  is  OPT = 10  on  *MAT_SPOTWELD.    It  is  available  for  spot  welds 
consisting  of  beam  elements,  solid  elements,  or  solid  assemblies.    Furthermore,  *DE-
FINE_SPOTWELD_FAILURE  requires  that  the  weld  nodes  be  tied  to  shell  elements 
using  tied  constraint  based  contact  options:  For  beam  element  welds,  only  *CON-
TACT_SPOTWELD  is  valid.    For  solid  element  welds  or  solid  assembly  welds,  valid 
options are the following. 
*CONTACT_TIED_SURFACE_TO_SURFACE 
*CONTACT_SPOTWELD 
*CONTACT_TIED_SHELL_EDGE_TO_SURFACE 
Other tied contact types cannot be used. 
The ADD keyword option adds materials to a previously defined spot weld failure data 
set. 
Data Card 1.  This card contains the data set’s ID and the first 7 parameters.  When the 
ADD option is active leave the 7 parameters blank. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
TFLAG 
DC1 
DC2 
DC3 
DC4 
EXN 
EXS 
Type 
I 
Default 
none 
I 
0 
F 
F 
F 
F 
F 
F 
1.183 
0.002963 0.0458 
0.1 
1.51 
1.51
Data Card 2.  .  This card contains 3 spot weld failure data parameters.  Do not include 
this card when the ADD option is active 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NAVG 
D_SN 
D_SS 
R_SULT 
Type 
Default 
I 
0 
F 
F 
F 
none 
none 
0.0 
Material-Specific Strength Data Cards.  Include one card for each material associated 
with the data set.  The next keyword (“*”) card terminates the keyword. 
4 
5 
6 
7 
8 
  Card 3 
1 
Variable 
MID 
Type 
I 
2 
SN 
F 
3 
SS 
F 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION
ID 
Identification  number  of  data  set,  input  as  FVAL  on  *MAT_-
SPOTWELD 
TFLAG 
Thickness flag for nominal stress calculation 
EQ.0:  Use minimum thickness 
EQ.1: Use average thickness 
Dynamic coefficient, 𝑐1 
Dynamic coefficient, 𝑐2 
Dynamic coefficient, 𝑐3 
Dynamic coefficient, 𝑐4 
Exponent on the normal term, 𝑛𝑛 
Exponent on the shear term, 𝑛𝑠 
DC1 
DC2 
DC3 
DC4 
EXN 
EXS
*DEFINE_SPOTWELD_FAILURE 
DESCRIPTION
NAVG 
Number of points in the time average of the load rates 
D_SN 
D_SS 
Default value of the static normal strength, 𝑆𝑛,stat 
Default value of the static shear strength, 𝑆𝑠,stat 
R_SULT 
Reference ultimate strength  
MID 
Material ID number of welded shell material 
Static normal strength of material MID. 𝑆𝑛,stat 
Static shear strength of material MID, 𝑆𝑠,stat 
SN 
SS 
Remarks: 
This  stress  based  failure  model,  which  was  developed  by  Lee  and  Balur  (2011),  uses 
nominal stress in the numerator and dynamical strengths in the denominator.  The weld 
fails when the stresses are outside of the failure surface defined as 
(
𝑠𝑛
𝑆𝑛,dyn
𝑛𝑛
)
+ (
𝑠𝑠
S𝑠,dyn
𝑛𝑠
)
= 1 
where 𝑠𝑛 and 𝑠𝑠 are nominal stress in the normal and tangential directions such that 
𝑠𝑛 =
𝑠𝑠 =
𝑃𝑛
𝐷𝑡
𝑃𝑠
𝐷𝑡
. 
𝑃𝑛 and 𝑃𝑠 are the loads carried by the weld in the normal and tangential directions, 𝐷is 
the  weld  diameter,  and  𝑡  is  the  thickness  of  the  welded  sheets.    If  the  sheets  have 
different thicknesses, then TFLAG controls whether the minimum or average thickness 
is used.  The dynamical strength terms in the denominator are load-rate dependent and 
are derived from static strength: 
𝑆𝑛,dyn = 𝑆𝑛,stat [𝑐1 + 𝑐2 (
) + 𝑐3 log (
)] 
𝑆𝑠,dyn = 𝑆𝑠,stat [𝑐1 + 𝑐2 (
) + 𝑐3log (
)] 
𝑃̇𝑛
𝑐4
𝑃̇𝑠
𝑐4
𝑃̇𝑛
𝑐4
𝑃̇𝑠
𝑐4
where  the  constants  𝑐1  to  𝑐4  are  the  input  in  the  fields  DC1  to  DC4, 𝑃̇𝑛  and  𝑃̇𝑠  are  the 
load  rates,  and  𝑆𝑛,stat  and  𝑆𝑠,stat  are  the  static  strengths  of  the  welded  sheet  materials 
which for each material are input using SN and SS.
When  two  different  materials  are  welded,  the  material  having  the  smaller  normal 
strength determines the strengths used for the weld.  Materials that do not have SN and 
SS values default to D_SN and D_SS from card 1.  The default values for DC1 to DC4, 
and  EXN  and  EXS  are  based  on  the  work  Chao,  Wang,  Miller  and  Zhu  (2010).    and 
Wang,  Chao,  Zhu,  and  Miller  (2010).    These  parameters  are  unitless  except  for  DC4 
which has units of force per unit time.  The default value of 0.1 is for MN/sec. 
The load rate, 𝑃̇, can be time averaged to reduce the effect of high frequency oscillations 
on the dynamic weld strength.  NAVG is the number of terms in the time average. 
If  R_SULT  is  defined  on  Card  2  and  the  PID  keyword  option  is  not  used,  then  D_SN 
and D_SS are interpreted to be reference values of the normal and shear static strength, 
and the SN field on Card 3 is interpreted as a material specific ultimate strength.  These 
values are then use to calculate material specific strength values by 
𝑆𝑛,𝑠𝑡𝑎𝑡 = 𝑆𝑛,𝑟𝑒𝑓 (
𝑆𝑢
𝑆𝑢,𝑟𝑒𝑓
) 
𝑆𝑠,𝑠𝑡𝑎𝑡 = 𝑆𝑠,𝑟𝑒𝑓 (
𝑆𝑢
𝑆𝑢,𝑟𝑒𝑓
) 
where 𝑆𝑛,𝑟𝑒𝑓 , 𝑆𝑠,𝑟𝑒𝑓 , and 𝑆𝑢,𝑟𝑒𝑓 , are D_SN, D_SS, and R_SULT  on card 2, and  𝑆𝑢 is SN on 
card 3.  With this option, the SS values are ignored.  If the PID keyword option is used, 
then  R_SULT is ignored and SN and SS are the static strength values.
*DEFINE_SPOTWELD_FAILURE_RESULTANTS 
Purpose:    Define  failure  criteria  between  part  pairs  for  predicting  spot  weld  failure.  
This  table  is  implemented  for  solid  element  spot  welds,  which  are  used  with  the  tied, 
constraint  based,  contact  option:  *CONTACT_TIED_SURFACE_TO_SURFACE.    Note 
that other tied contact types cannot be used.  The input in this section continues until then 
next  “*”  card  is  encountered.    Default  values  are  used  for  any  part  ID  pair  that  is  not 
defined.  Only one table can defined.  See *MAT_SPOTWELD where this option is used 
whenever OPT = 7. 
  Card 1 
Variable 
Type 
Default 
1 
ID 
I 
0 
2 
3 
4 
5 
6 
7 
8 
DSN 
DSS 
DLCIDSN DLCIDSS 
F 
F 
0.0 
0.0 
I 
0 
I 
0 
Failure Cards.  Provide as many as necessary.  The next keyword (“*”) card terminates 
the table definition.  
Card 2… 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID_I 
PID_J 
SNIJ 
SSIJ 
LCIDSNIJ
LCIDSSIJ 
Type 
I 
I 
F 
F 
Default 
none 
none 
0.0 
0.0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
ID 
DSN 
DSS 
DLCIDSN 
Identification number.  Only one table is allowed. 
Default value of the normal static stress at failure. 
Default value of the transverse static stress at failure. 
Load  curve  ID  defining  a  scale  factor  for  the  normal  stress  as  a
function  of  strain  rate.    This  factor  multiplies  DSN  to  obtain  the
failure value at a given strain rate.
DESCRIPTION
Load  curve  ID  defining  a  scale  factor  for  static  shear  stress  as  a 
function  of  strain  rate.    This  factor  multiplies  DSN  to  obtain  the
failure value at a given strain rate. 
Part ID I. 
Part ID J. 
The  maximum  axial  stress  at  failure  between  parts  I  and  J.    The
axial  stress  is  computed  from  the  solid  element  stress  resultants,
which are based on the nodal point forces of the solid element. 
The  maximum  shear  stress  at  failure  between  parts  I  and  J.    The 
shear stress is computed from the solid element stress resultants,
which are based on the nodal point forces of the solid element. 
Load  curve  ID  defining  a  scale  factor  for  the  normal  stress  as  a
function  of  strain  rate.    This  factor  multiplies  SNIJ  to  obtain  the 
failure value at a given strain rate. 
Load  curve  ID  defining  a  scale  factor  for  static  shear  stress  as  a
function  of  strain  rate.    This  factor  multiplies  SSIJ  to  obtain  the
failure value at a given strain rate. 
  VARIABLE   
DLCIDSS 
PID_I 
PID_J 
SNIJ 
DSSIJ 
LCIDSNIJ 
LCIDSSIJ 
Remarks: 
The stress based failure model, which was developed by Toyota Motor Corporation, is a 
function  of  the  peak  axial  and  transverse  shear  stresses.      The  entire  weld  fails  if  the 
stresses are outside of the failure surface defined by: 
(
𝜎𝑟𝑟
𝐹 )
𝜎𝑟𝑟
+ (
𝜏𝐹)
− 1 = 0 
𝐹   and  𝜏𝐹  are  specified  in  the  above  table  by  part  ID  pairs.    LS-DYNA 
where  𝜎𝑟𝑟
automatically  identifies  the  part  ID  of  the  attached  shell  element  for  each  node  of  the 
spot weld solid and checks for failure.  If failure is detected the solid element is deleted 
from the calculation. 
If the effects of strain rate are considered, then the failure criteria becomes: 
𝜎𝑟𝑟
[
𝐹 ]
𝑓𝑑𝑠𝑛(𝜀̇𝑝)𝜎𝑟𝑟
+ [
𝑓𝑑𝑠𝑠(𝜀̇𝑝)𝜏𝐹]
− 1 = 0
*DEFINE_SPOTWELD_MULTISCALE 
Purpose:  Associate beam sets with multi-scale spot weld types for modeling spot weld 
failure via the multi-scale spot weld method. 
Spot Weld/Beam Set Association Cards.  Provide as many cards as necessary.  This 
input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TYPE 
BSET 
TYPE 
BSET 
TYPE 
BSET 
TYPE 
BSET 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
MULTISCALE  spot  weld  type  to  use. 
SPOTWELD_MULTISCALE 
  See  *INCLUDE_-
Beam  set  which  uses  this  multi-scale  spot  weld  type  for  failure 
modeling. 
TYPE 
BSET 
Remarks: 
See  *INCLUDE_MULTISCALE_SPOTWELD  for  a  detailed  explanation  of 
capability.
this
*DEFINE_SPOTWELD_RUPTURE_PARAMETER 
Purpose:  Define a parameter by part ID for shell elements attached to spot weld beam 
elements using the constrained contact option: *CONTACT_SPOTWELD.  This table will 
not work with other contact types.  Only one table is permitted in the problem definition.  
Data, which is defined in this table, is used by the stress based spot weld failure model 
developed  by  Toyota  Motor  Corporation.    See  *MAT_SPOTWELD  where  this  option  is 
activated by setting the parameter OPT to a value of 9.  This spot weld failure model is a 
development of Toyota Motor Corporation. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
Type 
I 
Default 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
C11 
C12 
C13 
N11 
N12 
N13 
SIG_PF 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
  Card 3 
1 
2 
3 
Variable 
C21 
C22 
C23 
Type 
F 
F 
F 
4 
N2 
F 
Default 
5 
6 
7 
8 
SIG_NF
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCDPA 
LCDPM 
LCDPS 
LCDNA 
LCDNM 
LCDNS 
NSMT 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
PID 
Part ID for the attached shell. 
C11-N2 
Parameters for model, see Remarks below. 
Nugget pull-out stress, σP. 
Nugget fracture stress, σF. 
Curve  ID  defining  dynamic  scale  factor  of  spot  weld  axial  load
rate for nugget pull-out mode. 
Curve  ID  defining  dynamic  scale  factor  of  spot  weld  moment
load rate for nugget pull-out mode. 
Curve  ID  defining  dynamic  scale  factor  of  spot  weld  shear  load
rate for nugget pull-out mode. 
Curve  ID  defining  dynamic  scale  factor  of  spot  weld  axial  load
rate for nugget fracture mode. 
Curve  ID  defining  dynamic  scale  factor  of  spot  weld  moment
load rate for nugget fracture mode. 
Curve  ID  defining  dynamic  scale  factor  of  spot  weld  shear  load
rate for nugget fracture mode. 
The  number  of  time  steps  used  for  averaging  the  resultant  rates
for the dynamic scale factors. 
SIG_PF 
SIG_NF 
LCDPA 
LCDPM 
LCDPS 
LCDNA 
LCDNM 
LCDNS 
NSMT 
Remarks: 
This  failure  model  incorporates  two  failure  functions,  one  for  nugget  pull-out  and  the 
other for nugget fracture.  The nugget pull-out failure function is
𝐹𝑝 =
C11× 𝐴
𝐷N12 + C13 × 𝑆
𝐷N13
𝐷N11 + C12× 𝑀
𝜎𝑃 [1 + (𝜀̇𝑝
𝑝⁄
]
)
where A, M, and S are the axial force, moment, and shear resultants respectively, D is 
the  spot  weld  diameter,  and  the  Cowper-Symonds  coefficients  are  from  the  attached 
shell  material  model.    If  the  Cowper-Symonds  coefficients  aren’t  specified,  the  term 
within the square brackets, [ ], is 1.0.  The fracture failure function is 
𝐹𝑛 =
√(C21 × 𝐴 + C22 × 𝑀)2 + 3(C23 × 𝑆)2
𝐷N2𝜎𝐹 [1 + (𝜀̇𝑝
)
𝑝⁄
]
. 
When the load curves for the rate effects are specified, the failure criteria are  
C11 × 𝑓dpa(𝐴̇) × 𝐴
𝐷N11 + 𝐶12 × 𝑓dpa(𝑀̇ ) × 𝑀
𝐷N12 + C13 × 𝑓dpa(𝑆̇) × 𝑆
𝐷N13
𝜎𝑃
√[C21 × 𝑓dna(𝐴̇) × 𝐴 + C22 × 𝑓dnm(𝑀̇ ) × 𝑀]
+ 3[C23 × 𝑓𝑑𝑛𝑠(𝑆̇) × 𝑆]
𝐷N2𝜎𝐹
𝐹𝑝 =
𝐹𝑛 =
where f is the appropriate load curve scale factor.  The scale factor for each term is set to 
1.0 for when no load curve is specified.  No extrapolation is performed if the rates fall 
outside  of  the  range  specified  in  the  load  curve  to  avoid  negative  scale  factors.    A 
negative  load  curve  ID  designates  that  the  curve  abscissa  is  the  log10  of  the  resultant 
rate.    This  option  is  recommended  when  the  curve  data  covers  several  orders  of 
magnitude in the resultant rate.  Note that the load curve dynamic scaling replaces the 
Cowper-Symonds model for rate effects.  
Failure occurs when either of the failure functions is greater than 1.0.
*DEFINE_SPOTWELD_RUPTURE_STRESS 
Purpose:  Define a static stress rupture table by part ID for shell elements connected to 
spot  weld  beam  elements  using  the  constrained  contact  option:  *CONTACT_-
SPOTWELD.  This table will not work with other contact types.  Only one table is permitted 
in  the  problem  definition.    Data,  which  is  defined  in  this  table,  is  used  by  the  stress 
based  spot  weld  failure  model  developed  by  Toyota  Motor  Corporation.    See  *MAT_-
SPOTWELD where this option is activated by setting the parameter OPT to a value of 6. 
Part  Cards.    Define  rupture  stresses  part  by  part.      The  next  keyword  (“*”)  card 
terminates this input.  
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
SRSIG 
SIGTAU 
ALPHA 
Type 
I 
F 
F 
F 
  VARIABLE   
DESCRIPTION
PID 
SRSIG 
Part ID for the attached shell. 
𝐹 . 
Axial (normal) rupture stress, 𝜎𝑟𝑟
SRTAU 
Transverse (shear) rupture stress, 𝜏𝐹. 
ALPHA 
Scaling  factor  for  the  axial  stress  as  defined  by  Toyota.    The
default value is 1.0. 
Remarks: 
The stress based failure model, which was developed by Toyota Motor Corporation, is a 
function  of  the  peak  axial  and  transverse  shear  stresses.    The  entire  weld  fails  if  the 
stresses are outside of the failure surface defined by: 
(
𝜎𝑟𝑟
𝐹 )
𝜎𝑟𝑟
+ (
𝜏𝐹)
− 1 = 0 
𝐹  and 𝜏𝐹 are specified in the above table by part ID.  LS-DYNA automatically 
where 𝜎𝑟𝑟
identifies the part ID of the attached shell element for each node of the spot weld beam 
and independently checks each end for failure.  If failure is detected in the end attached 
to  the  shell  with  the  greatest  plastic  strain,  the  beam  element  is  deleted  from  the 
calculation. 
If the effects of strain rate are considered, then the failure criteria becomes:
[
𝜎𝑟𝑟
]
𝐹 (𝜀̇𝑝)
𝜎𝑟𝑟
+ [
]
𝜏𝐹(𝜀̇𝑝)
− 1 = 0 
𝐹 (𝜀̇𝑝) and  𝜏𝐹(𝜀̇𝑝)  are found by using the Cowper and Symonds model which 
where 𝜎𝑟𝑟
scales the static failure stresses: 
𝜎𝑟𝑟
𝐹 (𝜀̇𝑝) = 𝜎𝑟𝑟
𝜀̇𝑝
⎡1 + (
⎢
⎣
𝑝⁄
)
⎤ 
⎥
⎦
𝑝⁄
𝜀̇𝑝
𝜏𝐹(𝜀̇𝑝) = 𝜏𝐹
⎡1 + (
⎢
⎣
where  𝜀̇𝑝is  the  average  plastic  strain  rate  which  is  integrated  over  the  domain  of  the 
attached  shell  element,  and  the  constants  p  and  C  are  uniquely  defined  at  each  end  of 
the beam element by the constitutive data of the attached shell.   The constitutive model 
is  described  in  the  material  section  under  keyword:  *MAT_PIECEWISE_LINEAR_-
PLASTICITY. 
⎤ 
⎥
⎦
)
The peak stresses are calculated from the resultants using simple beam theory. 
𝜎𝑟𝑟 =
𝑁𝑟𝑟
+
√𝑀𝑟𝑠
2 + 𝑀𝑟𝑡
𝛼𝑍
𝜏 =
𝑀𝑟𝑟
2𝑍
+
2 + 𝑁𝑟𝑡
√𝑁𝑟𝑠
where the area and section modulus are given by: 
𝐴 = 𝜋
𝑍 = 𝜋
𝑑2
𝑑3
32
and d is the diameter of the spot weld beam.
*DEFINE_STAGED_CONSTRUCTION_PART_{OPTION} 
Available options include: 
<BLANK> 
SET 
Purpose:    Staged  construction.    This  keyword  offers  a  simple  way  to  define  parts  that 
are  removed  (e.g.,  during  excavation),  added  (e.g.,  new  construction)  and  used 
temporarily  (e.g.,  props)  during  the  analysis.    Available  for  solid,  shell,  and  beam 
element parts.  
Part Cards.  Provide as many as necessary.  This input ends at the next keyword (“*”) 
card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID/PSID 
STGA 
STGR 
Type 
I 
I 
I 
Default 
none 
See 
Remark
s 
See 
Remark
s 
  VARIABLE   
DESCRIPTION
Part ID (or Part Set ID for the_SET option) 
Construction stage at which part is added 
Construction stage at which part is removed 
PID 
STGA 
STGR 
Remarks: 
Used with *DEFINE_CONSTRUCTION_STAGES (defines the meaning of stages STGA 
and  STGR)  and  *CONTROL_STAGED_CONSTRUCTION.    If  STGA = 0,  the  part  is 
present at the start of the analysis.  If STGR = 0, the part is still present at the end of the 
analysis.  Examples: 
1.  Soil that is excavated would have STGA = 0 but STGR > 0 
2.  New construction would have STGA > 0 and STGR = 0
3.  Temporary works would have STGA > 0, STGR > STGA. 
This  is  a  convenience  feature  that  reduces  the  amount  of  input  data  needed  for  many 
typical construction models.  Internally, LS-DYNA checks for *LOAD_REMOVE_PART, 
*LOAD_GRAVITY_PART  and  *LOAD_STIFFEN_PART  referencing  the  same  PID.  
Generally,  these  will  not  be  present  and  LS-DYNA  creates  the  data  using  STGA  and 
STGR,  and  default  gravity  and  pre-construction  stiffness  factor  from  *CONTROL_-
STAGED_CONSTRUCTION.  If existing cards are found, STGA and STGR are inserted 
into  the  existing  data.    During  the  analysis,  any  load  curves  entered  on  those  existing 
cards will override STGA and STGR.
*DEFINE_STOCHASTIC_ELEMENT_OPTION 
Options: 
  SOLID_VARIATON for solid elements. 
  SHELL_VARIATION for shell elements. 
Purpose:    Define  the  stochastic  variation  in  the  yield  stress,  damage/failure  models, 
density,  and  elastic  moduli  for  solid  material  models  with  the  STOCHASTIC  option, 
currently materials 10, 15, 24, 81, and 98.  This option overrides values assigned by *DE-
FINE_STOCHASTIC_VARIATION. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IDE 
VARSY 
VARF 
VARRO 
VARE 
Type 
Default 
I 
0 
F 
0 
F 
0 
F 
0 
F 
0 
  VARIABLE   
DESCRIPTION
IDE 
Element ID 
VARSY 
VARF 
VARRO 
VARE 
The  yield  stress  and  its  hardening  function  are  scaled  by
1.+VARSY. 
The failure criterion is scaled by 1+VARF 
The  density  is  scaled  by  1+VARRO.   This  is  intended  to  be  used
with topology optimization.  This option is not available for shell
elements. 
The elastic moduli are scaled by 1+VARE.  This is intended to be
used with topology optimization.
*DEFINE_STOCHASTIC_VARIATION 
Purpose:  Define the stochastic variation in the yield stress and damage/failure models 
for  material  models  with  the  STOCHASTIC  option,  currently  materials  10,  15,  24,  81, 
and 98 and the shell version of material 123. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ID_SV 
PID 
PID_TYP 
ICOR 
VAR_S 
VAR_F 
IRNG 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
Yield Stress Card for Built-in Distribution.  Card 2 for VAR_S set to 0, 1, or 2. 
4 
5 
6 
7 
8 
  Card 2 
Variable 
1 
R1 
Type 
F 
2 
R2 
F 
3 
R3 
F 
Default 
Yield Stress Card for Load Curve.  Card 2 for VAR_S set to 3 or 4. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
Type 
Default 
I
Failure Strain Card for Built-in Distribution.  Card 2 for VAR_F set to 0, 1, or 2. 
4 
5 
6 
7 
8 
  Card 2 
Variable 
1 
R1 
Type 
F 
2 
R2 
F 
3 
R3 
F 
Default 
Failure Strain Card for Load Curve.  Card 2 for VAR_F set to 3 or 4. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
Type 
Default 
I 
0 
  VARIABLE   
DESCRIPTION
ID_SV 
Stochastic variation ID.  A unique ID number must be used. 
PID 
*PART ID or *SET_PART ID. 
PID_TYP 
Flag  for  PID  type.    If  PID  and  PID_TYP  are  both  0,  then  the 
properties  defined  here  apply  to  all  shell  and  solid  parts  using
materials with the STOCHASTIC option. 
EQ.0: PID is a *PART ID. 
EQ.1: PID is a *SET_PART ID 
ICOR 
Correlation between the yield stress and failure strain scaling. 
EQ.0: Perfect correlation. 
EQ.1:  No  correlation.    The  yield  stress  and  failure  strain  are
independently scaled.
VARIABLE   
DESCRIPTION
VAR_S 
Variation type for scaling the yield stress.  
EQ.0: The scale factor is 1.0 everywhere. 
EQ.1: The  scale  factor  is  random  number  in  the  uniform
random  distribution  in  the  interval  defined  by  R1  and
R2. 
EQ.2: The  scale  factor  is  a  random  number  obeying  the
Gaussian distribution defined by R1, R2, and R3.  
EQ.3: The scale factor is defined by the probability distribution
function defined by curve  LCID. 
EQ.4: The scale factor is defined by the cumulative distribution 
function defined by curve LCID.  
VAR_F 
Variation type for scaling failure strain.  
EQ.0: The scale factor is 1.0 everywhere. 
EQ.1: The  scale  factor  is  random  number  in  the  uniform
random  distribution  in  the  interval  defined  by  R1  and
R2. 
EQ.2: The  scale  factor  is  a  random  number  obeying  the
Gaussian distribution defined by R1, R2, and R3.  
EQ.3: The scale factor is defined by the probability distribution
function defined by curve  LCID. 
EQ.4: The scale factor is defined by the cumulative distribution 
function defined by curve LCID.  
IRNG 
Flag for random number generation. 
EQ.0: Use  deterministic  (pseudo-)  random  number  generator. 
The same input always leads to the same distribution. 
EQ.1: Use  non-deterministic  (true)  random  number  generator.
With the same input, a different distribution is achieved
in each run. 
R1, R2, R3 
Real values to define the stochastic distribution.  See below. 
LCID 
Curve ID defining the stochastic distribution.  See below.
*DEFINE_STOCHASTIC_VARIATION 
Each  integration  point  𝑥𝑔  in  the  parts  specifed  by  PID  is  assigned  the  random  scale 
factors 𝑅𝑆 and 𝑅𝐹 that are applied to the values calculated by the material model for the 
yield stress and failure strain.  
𝜎𝑦 = 𝑅𝑠(𝑥𝑔)𝜎𝑦(𝜀̅𝑝, … ) 
𝜀̅FAIL
= 𝑅𝐹(𝑥𝑔)𝜀̅FAIL
(𝜀̇, 𝜀̅𝑝, … ) 
The  scale  factors  vary  spatially  over  the  model  according  to  the  chosen  statistical 
distributions defined in this section and are independent of time.  The scale factors may 
be  completely  correlated  or  uncorrelated  with  the  default  being  completely  correlated 
since  the  failure  strain  is  generally  reduced  as  the  yield  stress  increases.    The  scale 
factors 𝑅𝑆 and 𝑅𝐹 may be stored as extra history variables as follows:   
Material Model 
10 
15 
24 
81 
98 
123 (shells only) 
History Variable #  for RS
5 
7 
6 
6 
7 
6 
History Variable #  for RF
6 
8 
7 
7 
8 
7 
The  user  is  responsible  for  defining  the  distributions  so  that  they  are  physically 
meaningful and are restricted to a realistic range.  Since neither the yield stress nor the 
failure  strain  may  be  negative,  for  example,  the  minimum  values  of  the  distributions 
must always be greater than zero. 
The  probability  that  a  particular  value  𝑅  will  occur  defines  the  probability  distribution 
function, 𝑃(𝑅). Since a value must be chosen from the distribution, the integral from the 
minimum to the maximum value of 𝑅 of the probability distribution function must be 
1.0, 
𝑅MAX
∫
𝑅MIN
𝑃(𝑅)𝑑𝑅 = 1
. 
Another  way  to  characterize  a  distribution  is  the  cumulative  distribution  function  𝐶(𝑅) 
which defines the probability that a value will lie between 𝑅𝑀𝐼𝑁 and 𝑅, 
𝐶(𝑅) = ∫
𝑅MIN
𝑃(𝑅̂ )𝑑𝑅̂
. 
By  definition  𝐶(𝑅𝑀𝐼𝑁) = 0  and    𝐶(𝑅𝑀𝐴𝑋) = 1.  An  inverse  cumulative  probability 
function D gives the number for a cumulative probability of 𝐶(𝑅), 
𝐷(𝐶(𝑅)) = 𝑅.
A  random  varriable  satisfying  the  probability  distribution  function  P(R)  can  be 
generated from a sequence of uniformly distributed numbers, 𝑅̂ 𝐼, for 𝐼 = 1, 𝑁, using the 
inverse cumulative distribution function 𝐷 as  
𝑅𝐼 = 𝐷(𝑅̂ 𝐼). 
The scale factors for the yield stress and the failure strain may  be  generated using the 
same  value  of  𝑅̂ 𝐼  for  both  (ICOR = 0)  or  by  using  independent  values  each  one 
(ICOR = 1).    If  the  same  values  are  used,  there  is  perfect  correlation,  and  the  failure 
strain scale factor becomes an implicit value of yield stress scale factor. 
VAR = 0.  No Scaling. 
The corresponding yield stress or failure strain is not scaled. 
VAR = 1.  Scaling from Uniform Distribution 
A  uniform  distribution  is  specified  by  setting  VAR = 1.    The  input  variable  R1  is 
interpreted  as  𝑅MIN  and  R2  as  𝑅MAX.  If  R1 = R2,  then  the  yield  stress  or  failure  strain 
will be scaled by R1. 
When  using  the  uniform  random  distribution,  the  probability  of  a  particular  value  is 
given by 
and the cumulative probability function is given by 
𝑃(𝑅) =
𝑅MAX − 𝑅MIN
𝐶(𝑅) =
𝑅 − 𝑅MIN
𝑅MAX − 𝑅MIN
. 
VAR = 2.  Gaussian Distribution 
The  Gaussian  distribution,  VAR = 2,  is  smoothly  varying  with  a  peak  at  µ  and  63 
percent  of  the  values  occurring  within  the  interval  of  one  standard  deviation 𝜎, 
[𝜇 − 𝜎, 𝜇 + 𝜎].    The  input  parameter  R1  is  interpreted  as  the  mean, 𝜇,,  while  R2  is 
interpreted as the standard deviation, 𝜎.  There is a finite probability that the values of 
𝑅 will be outside of the range that are physically meaningful in the scaling process, and 
R3  which  is  interpreted  as  𝛿  restricts  the  range  of  R  to  [𝜇 − 𝛿, 𝜇 + 𝛿]  The  resulting 
truncated Gaussian distribution is rescaled such that, 
𝐷(𝜇 + 𝛿) = 1.
VAR = 3 or 4.  Distribution from a Load Curve 
The  user  may  directly  specify  the  probability  distribution  function  or  the  cumulative 
probability  distribution  function  with  *DEFINE_CURVE  by  setting  VAR = 3  or 
VAR = 4, respectively, and then specifying the required curve ID on the next data card.  
Stochastic  variations  may  be  used  simultaneously  with  the  heat  affected  zone  (HAZ) 
options in LS-DYNA .  The effect of the scale factors 
from  stochastic  variation  and  HAZ  options  are  multiplied  together  to  scale  the  yield 
stress and failure strain, 
𝜎𝑦 = 𝑅𝑆(𝑥𝑔)𝑅𝑆
𝜀̅FAIL
= 𝑅𝐹(𝑥𝑔)𝑅𝐹
HAZ𝜎𝑦(𝜀̅𝑝, … ) 
HAZ𝜀̅FAIL
(𝜀̇, 𝜀̅𝑝, … ).
*DEFINE 
Purpose:  To interpolate from point data a continuously indexed family of nonintersect-
ing  curves.    The  family  of  curves,  ℱ ,  consists  of  x-y  curves,  𝑓𝑠(𝑥),  indexed  by  a 
parameter, 𝑠. 
ℱ = {𝑓𝑠(𝑥)∣∀𝑠 ∈ [𝑠min, 𝑠max]}. 
The interpolation is built up by sampling functions in ℱ  at discrete parameter values, 𝑠𝑖, 
𝑓𝑠𝑖(𝑥) ∈ ℱ . 
The  points,  𝑠𝑖,  are  input  to  LS-DYNA  on  the  data  cards  for  the  *DEFINE_TABLE 
keyword.  LS-DYNA requires that they be ordered from least to greatest.  The curves, 
𝑓𝑠𝑖(𝑥), must be defined as lists of (𝑥, 𝑦) pairs in a collection of *DEFINE_CURVE sections 
that  directly  follow  the  *DEFINE_TABLE  section.    Each  *DEFINE_CURVE  section  is 
paired to its corresponding 𝑠𝑖 value by list position (and not load curve ID, for that see 
*DEFINE_TABLE_2D). 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TBID 
SFA 
OFFA 
Type 
I 
F 
Default 
none 
1. 
F 
0. 
Points Cards.  Place one point per card.  The values must be in ascending order.  Input 
is terminated when a “*DEFINE_CURVE” keyword card is found.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VALUE 
Type 
F 
Default 
0.0 
Include one *DEFINE_CURVE input section here for each point defined above.  The 𝑖th 
*DEFINE_CURVE card contains the curve at the 𝑖th *DEFINE_TABLE value.
TBID 
*DEFINE_TABLE 
DESCRIPTION
Table  ID.    Tables  and  Load  curves  may  not  share  common  ID's.
LS-DYNA  allows  load  curve  ID's  and  table  ID's  to  be  used
interchangeably.   
SFA 
Scale factor for VALUE. 
OFFA 
Offset for VALUE, see explanation below. 
VALUE 
Load curve will be defined corresponding to this value, e.g., this 
value could be a strain rate, see purpose above. 
Motivation: 
This  capability  was  implemented  with  strain-rate  dependent  stress-strain  relations  in 
mind.    To  define  such  a  function,  the  first  step  is  to  tabulate  stress-strain  curves  at 
known strain-rate values.  Then, the list of strain-rates is written in ascending order to 
the data cards following *DEFINE_TABLE.  Following *DEFINE_TABLE, the tabulated 
stress-strain  curves  must  be  input  to  LS-DYNA  as  a  set  of  *DEFINE_CURVE  sections 
ordered  so  that  the  𝑖th  curve  corresponds  to  the    𝑖th  strain-rate  point.    This  section  is 
structured as: 
*DEFINE_TABLE 
strain-rate point 1 
strain-rate point 2 
⋮  
strain-rate point n 
*DEFINE_CURVE 
[stress-strain curve at strain-rate 1] 
*DEFINE_CURVE 
[stress-strain curve at strain-rate 2] 
⋮  
*DEFINE_CURVE 
[stress-strain curve at strain-rate n] 
Details, Features and Limitations: 
1.  All the curves in a table must start from the same abscissa value and end at the 
same  abscissa  value.    This  limitation  is  necessary  to  avoid  slow  indirect  ad-
dressing  in  the  inner  loops  used  in  the  constitutive  model  stress  evaluation.  
Curves must not intersect except at the origin and end points.
2.  Each curve may have unique spacing and an arbitrary number of points in its 
definition. 
3.  All the curves in a table must share the same value of LCINT. 
4. 
In most applications, curves can only be extrapolated in one direction, that is, to 
the right of the last data point.  An example would be curves representing effec-
tive  stress  vs.    effective  plastic  strain.    For  cases  when  extrapolation  is  only  to 
the  right,  the  curves  comprising  a  table  are  allowed  to  intersect  only  at  their 
starting  point  but  the  curves  and  their  extrapolations  must  not  intersect  else-
where. 
For  other  applications  in  which  the  curves  are  extrapolated  in  both  directions, 
the  curves  and  their  extrapolations  are  not  allowed  to  intersect  except  at  the 
origin (0,0).  An example would be curves representing force vs.  change in gage 
length where negative values are compressive and positive values are tensile. 
5.  Load curve IDs defined for the table may be referenced elsewhere in the input. 
6.  No  keyword  commands  may  come  between  *DEFINE_TABLE  and  the  *DE-
FINE_CURVE  commands  that  feed  the  table.      The  set  of  *DEFINE_CURVE 
commands  must  not  be  interrupted  by  any other  keyword.    This  coupling  be-
tween  *DEFINE_TABLE  and  subsequent  *DEFINE_CURVE  commands  is  an 
exception to the general order-independence of the keyword format. 
7.  VALUE is scaled in the same manner as in *DEFINE_CURVE, i.e., 
Scaled value = SFA×(Defined value + OFFA). 
8.  Unless  stated  otherwise  in  the  description  of  a  keyword  command  that 
references  a  table,  there  is  no  extrapolation  beyond  the  range  of  VALUEs  de-
fined for the table.  For example, if the table VALUE represents strain rate and 
the  calculated  strain  rate  exceeds  the  last/highest  VALUE  given  by  the  table, 
the  stress-strain  curve  corresponding  to  the  last/highest  table  VALUE  will  be 
used.
*DEFINE_TABLE_2D 
Purpose:    Define  a  table.    Unlike  the  *DEFINE_TABLE  keyword  above,  a  curve  ID  is 
specified  for  each  value  defined  in  the  table.    This  allows  the  same  curve  ID  to  be 
referenced by multiple tables, and the curves may be defined anywhere in the input file.  
Other  than  these  differences  from  *DEFINE_TABLE,  the  general  rules  given  in  the 
remarks of *DEFINE_TABLE still apply. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TBID 
SFA 
OFFA 
Type 
I 
F 
Default 
none 
1. 
F 
0. 
Points Cards.  Place one point per card.  The values must be in ascending order.  Input 
is terminated when a “*DEFINE_CURVE” keyword card is found. 
  Card 2 
1 
2 
3 
4 
Variable 
VALUE 
CURVE ID 
Type 
F 
I 
Default 
0.0 
none 
  VARIABLE   
TBID 
DESCRIPTION
Table  ID.    Tables  and  Load  curves  may  not  share  common  ID's.
LS-DYNA  allows  load  curve  ID's  and  table  ID's  to  be  used
interchangeably.   
SFA 
Scale factor for VALUE. 
OFFA 
Offset for VALUE, see explanation below. 
VALUE 
Load  curve  will  be  defined  corresponding  to  this  value.    The
value could be, for example, a strain rate. 
CURVEID 
Load curve ID.  See Remark 1.
*DEFINE 
1.  Though  generally  of  no  concern  to  the  user,  curve  CURVEID  is  automatically 
duplicated  during  initialization  and  the  duplicate  curve  is  automatically  as-
signed  a  unique  curve  ID.    The  generated  curve  IDs  used  by  the  table  are  re-
vealed in d3hsp.  It is generally only necessary to know the generated curve IDs 
when interpreting warning messages about those curves.
*DEFINE_TABLE_3D 
Purpose:  Define a three dimensional table.  For each value defined below, a table ID is 
specified.    For  example,  in  a  thermally  dependent  material  model,  the  value  given 
below  could  correspond  to  temperature  for  a  table  ID  defining  effective  stress  versus 
strain curves for a set of strain rate values.  Each table ID can be referenced by multiple 
three dimensional tables, and the tables may be defined anywhere in the input.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TBID 
SFA 
OFFA 
Type 
I 
F 
Default 
none 
1. 
F 
0. 
Points Cards.  Place one point per card.  The values must be in ascending order.  Input 
is terminated when a “*DEFINE_CURVE” keyword card is found. 
  Card 2 
1 
2 
3 
4 
Variable 
VALUE 
TABLE ID 
Type 
F 
I 
Default 
0.0 
none 
  VARIABLE   
TBID 
DESCRIPTION
Table  ID.    Tables  and  Load  curves  may  not  share  common  ID's.
LS-DYNA  allows  load  curve  ID's  and  table  ID's  to  be  used
interchangeably.   
SFA 
Scale factor for VALUE. 
OFFA 
Offset for VALUE, see explanation below. 
VALUE 
Load curve will be defined corresponding to this value, e.g., this
value could be a strain rate for example. 
TABLEID 
Table ID.
*DEFINE 
1.  VALUE is scaled in the same manner as in *DEFINE_CURVE, i.e., 
Scaled value = SFA × (Defined value  +  OFFA). 
2.  Unless  stated  otherwise  in  the  description  of  a  keyword  command  that 
references  a  table,  there  is  no  extrapolation  beyond  the  range  of  VALUEs  de-
fined for the table.  For example, if the table VALUE represents strain rate and 
the  calculated  strain  rate  exceeds  the  last/highest  VALUE  given  by  the  table, 
the  stress-strain  curve  corresponding  to  the  last/highest  table  VALUE  will  be 
used
*DEFINE_TABLE_MATRIX 
This  is  an  alternative  input  format  for  *DEFINE_TABLE  that  allows  for  reading  data 
from  an  unformatted  text  file  containing  a  matrix  with  data  separated  by  comma 
delimiters.  The purpose is to use data saved directly from excel sheets without having 
to convert it to keyword syntax.   
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TBID 
Type 
I 
FILENAME 
A70 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NROW 
NCOL 
SROW 
SCOL 
SVAL 
OROW 
OCOL 
OVAL 
Type 
I 
I 
F 
Default 
None 
None 
1. 
F 
1. 
F 
1. 
F 
0. 
F 
0. 
F 
0. 
  VARIABLE   
TBID 
DESCRIPTION
Table  ID.    Tables  and  Load  curves  may  not  share  common  ID's.
LS-DYNA  allows  load  curve  ID's  and  table  ID's  to  be  used
interchangeably.   
FILENAME 
Name of file containing table data (stored as a matrix). 
NROW 
Number of rows in the matrix, same as number of rows in the file
the 
FILENAME. 
interpretation  of  rows  and  columns  in  the  read  matrix,  see
remarks. 
  A  negative  value  of  NROW  switches 
NCOL 
Number of columns in the matrix, same as number of data entries
per row in the file FILENAME 
SROW 
Scale factor for row data, see remarks. 
SCOL 
SVAL 
15-268 (DEFINE) 
Scale factor for column data, see remarks.
VARIABLE   
DESCRIPTION
OROW 
Offset for row data, see remarks. 
Offset for column data, see remarks. 
Offset for matrix values, see remarks. 
OCOL 
OVAL 
Remarks: 
The  use  of  this  keyword  allows  for  inputting  a  table  in  form  of  a  matrix  from  a  file, 
exemplified here by a 4 × 5 matrix. 
C1 
V11 
V21 
V31 
⋮ 
C2 
V12 
V22 
V32 
⋮ 
C3 
V13 
V23 
V33 
⋮ 
C4 
V14 
V24 
V34 
⋮ 
R1 
R2 
R3 
⋮ 
The unformatted file representing this matrix would contain the following data 
,C1,C2,C3,C4 
R1,V11,V12,V13,V14 
R2,V21,V22,V23,V24 
R3,V31,V32,V33,V34 
Note that the first entry in the matrix is a dummy and delimited by an initial comma in 
the file.  The keyword card for this matrix is: (TBID = 1000 and the filename is file.txt) 
*DEFINE_TABLE_MATRIX 
1000,file.txt 
4,5 
This is equivalent to using: 
*DEFINE_TABLE 
1000 
C1 
C2 
C3 
C4 
*DEFINE_CURVE 
1001 
R1,V11 
R2,V21 
R3,V31 
*DEFINE_CURVE 
1002 
R1,V12
R2,V22 
R3,V32 
*DEFINE_CURVE 
1003 
R1,V13 
R2,V23 
R3,V33 
*DEFINE_CURVE 
1004 
R1,V14 
R2,V24 
R3,V34 
All  entries  in  the  matrix  can  be  scaled  and  offset  following  the  convention  for  other 
tables and curves: 
Scaled Value = S[ROW/COL] × (Value + O[ROW/COL]) 
Finally,  the  matrix  can  be  transposed  by  setting  NROW  to  a  negative  value.    In  the 
example above this would mean that 
*DEFINE_TABLE_MATRIX 
1000,file.txt 
-4,5 
is equivalent to using: 
*DEFINE_TABLE 
1000 
R1 
R2 
R3 
*DEFINE_CURVE 
1001 
C1,V11 
C2,V12 
C3,V13 
C4,V14 
*DEFINE_CURVE 
1002 
C1,V21 
C2,V22 
C3,V23 
C4,V24 
*DEFINE_CURVE 
1003 
C1,V31 
C2,V32 
C3,V33 
C4,V34
In this case, any scaling applies to the matrix entries before transposing the data, i.e., for 
row entries the scaled value is 
and for column entries 
Scaled Value = SROW × (𝑅 + OROW), 
Scaled Value = SCOL × (𝐶 + OCOL) 
regardless the sign of TBID.
*DEFINE_TARGET_BOUNDARY 
Purpose:  This keyword is used to define the desired boundary of a formed part.  This 
boundary  provides  the  criteria  used  during  blank-size  development.    The  definitions 
associated with this keyword are used, exclusively, by the *INTERFACE_BLANKSIZE_-
DEVELOPMENT feature. 
Point  Cards.    Include  one  card  for  each  point  in  the  curve.    These  points  are 
interpolated to form a closed curve.  This input is terminated with *END. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
X 
Y 
Z 
Type 
E16.0 
E16.0 
E16.0 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION
X, Y, Z 
Location coordinates of a target node. 
Remarks: 
1.  The  keyword  file  specified  on  the  second  data  card  for  the  *INTERFACE_-
BLANKSIZE_DEVELOPMENT  keyword  must  contain  a  *DEFINE_TARGET_-
BOUNDARY keyword. 
2.  A  partial  keyword  input  is  shown  below.    Note  that  the  input  is  in  a  3E16.0 
FORTRAN format.  Also note that the first and last curve points coincide. 
*KEYWORD 
*DEFINE_TARGET_BOUNDARY 
    -1.83355e+02    -5.94068e+02    -1.58639e+02 
    -1.80736e+02    -5.94071e+02    -1.58196e+02 
    -1.78126e+02    -5.94098e+02    -1.57813e+02 
    -1.75546e+02    -5.94096e+02    -1.57433e+02 
    -1.72888e+02    -5.94117e+02    -1.57026e+02 
           ⋮               ⋮               ⋮ 
    -1.83355e+02    -5.94068e+02    -1.58639e+02 
*END 
Typically, these boundary nodes obtained from the boundary curves for a final 
(trimmed) piece, or from a draw blank edge at a certain distance outside of the 
draw beads.  LS-PrePost 4.1 can generate the points for this keyword from IGES
data.  To use IGES data select Curve → Convert→ Method (To Keyword) → Select 
*DEFINE_TARGET_BOUNDARY;  pick  the  curves  then  select  “To  Key”.    To 
output a keyword choose File → Save as → Save Keyword As, and select “Out-
put Version” as “V971_R7”. 
3.  This feature is available in LS-DYNA R6 Revision 74560 and later releases.
*DEFINE_TRACER_PARTICLES_2D 
Purpose:  Define tracer particles that follow the deformation of a material.  This is useful 
for  visualizing  the  deformation  of  a  part  that  is  being  adapted  in  a  metal  forming 
operation.  Nodes used as tracer particles should only be used for visualization and not 
associated  with  anything  in  the  model  that  may  alter  the  response  of  the  model,  e.g., 
they should not be used in any elements except those with null materials. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSET 
PSET 
Type 
I 
Default 
none 
I 
0 
  VARIABLE   
DESCRIPTION
NSET 
PSET 
The node set ID for the nodes used as tracer particles. 
Optional  part  set  ID.    If  this  part  set  is  specified,  only  tracer
particles in these parts are updated and the others are stationary.
If this part set is not specified, all tracer particles are updated.
*DEFINE 
Purpose:    Define  a  transformation  for  the  INCLUDE_TRANSFORM  keyword  option.  
The  *DEFINE_TRANSFORMATION  command  must  be  defined  before  the  *IN-
CLUDE_TRANSFORM command can be used. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TRANID 
Type 
I 
Default 
none 
Transformation  Cards.    Include  as  many  cards  as  necessary.    This  input  ends  at  the 
next keyword (“*”) card. 
  Card 2 
1 
Variable 
OPTION 
Type 
A 
2 
A1 
F 
3 
A2 
F 
4 
A3 
F 
5 
A4 
F 
6 
A5 
F 
7 
A6 
F 
8 
A7 
F 
  VARIABLE   
DESCRIPTION
TRANID 
Transform ID. 
OPTION 
For the available options see the table below. 
A1-A7 
Parameters.  See Table 15-47 below for the available options.
OPTION 
PARAMETERS 
FUNCTION 
MIRROR 
a1, a2, a3, a4, a5, a6, a7  Reflect,  about  a  mirror  plane  defined  to 
its 
contain 
normal  pointing 
(a1, a2, a3) 
toward  (a4, a5, a6).    Setting  a7 = 1 reflects  the 
coordinate  system  as  well,  i.e.,  the  mirrored 
coordinate  system  uses  the  left-hand-rule  to 
determine the local 𝑧-axis. 
(a1, a2, a3)  having 
from  point 
the  point 
SCALE 
a1, a2, a3 
Scale  the  global  x,  y,  and  z  coordinates  of  a 
point by a1, a2, and a3, respectively.  If zero, a 
default of unity is set. 
ROTATE 
a1, a2, a3, a4, a5, a6, a7  Rotate through an angle (deg), a7, about a line 
with  direction  cosines  a1,  a2,  and  a3  passing 
through the point with coordinates a4, a5, and 
a6. 
TRANSL 
a1, a2, a3 
POINT 
a1,a2,a3,a4 
POS6P 
a1, a2, a3, a4, a5, a6 
POS6N 
a1, a2, a3, a4, a5, a6 
If  a4  through  a7  are  zero,  then  a1  and  a2  are 
the  ID’s  of  two  POINTs  and  a3  defines  the 
rotation angle.  The axis of rotation is defined 
by  a  vector  going  from  point  with  ID  a1  to 
point with ID a2.  
Translate the x, y, and z coordinates of a point 
by a1, a2, and a3, respectively. 
Define  a  point  with  ID,  a1,  with  the  initial 
coordinates a2, a3, and a4. 
Positioning  by  6  points.    Affine  transfor-
mation  (rotation  and  translation,  no  scaling) 
given by three start points a1, a2, and a3 and 
three  target  points  a4,  a5,  and  a6.    The  six 
POINTs  must  be  defined  before  they  are 
referenced.  Only 1 POS6P option is permitted 
within 
*DEFINE_TRANSFORMATION 
a 
definition. 
Positioning by 6 nodes.  Affine transformation 
(rotation and translation, no scaling) given by 
three  start  nodes  a1,  a2,  and  a3  and  three 
target  nodes  a4,  a5,  and  a6.    The  six  nodes 
must  be  defined  before  they  are  referenced.  
Only  1  POS6N  option  is  permitted  within  a
OPTION 
PARAMETERS 
FUNCTION 
*DEFINE_TRANSFORMATION definition. 
Table 15-47.  List of allowed transformations. 
Each  option  represents  a  transformation  matrix.    When  more  than  one  option  is  used, 
the  transformation  matrix  defined  by  MIRROR,  SCALE,  ROTATE  or  TRANSL  is 
applied to the previously defined existing matrix to form the new global transformation 
matrix.    Therefore  the  ordering  of  the  SCALE,  ROTATE,  and  TRANSL  commands  is 
important.  It is generally recommended to first scale, then rotate, and finally translate 
the  model.    POS6P  and  POS6N  differ  from  other  options  by  not  applying  their 
transformation matrix to the existing global matrix.  Instead the transformation matrix 
defined by POS6P or POS6N replaces the existing matrix and becomes the new global 
transformation matrix. 
The  POINT  option  in  ROTATE  provides  a  means  of  defining  rotations  about  axes 
defined  by  the  previous  transformations.    The  coordinates  of  the  two  POINTs  are 
transformed  by  all  the  transformations  up  to  the  transformation  where  they  are 
referenced.    The  POINTs  must  be  defined  before  they  are  referenced,  and  their 
identification  numbers  are  local  to  each  *DEFINE_TRANSFORMATION. 
  The 
coordinates  of  a  POINT  are  transformed  using  all  the  transformations  before  it  is 
referenced, not just the transformations between its definition and its reference.  To put 
it  another  way,  while  the  ordering  of  the  transformations  is  important,  the  ordering 
between the POINTs and the transformations is not important. 
NOTE:  When  *DEFINE_TRANSFORMATION 
is  called 
from  within  the  target  of  an  *INCLUDE_TRANS-
FORM    keyword,  the  result  will  involve  stacked 
transformations. 
In the following example, the *DEFINE_TRANSFORMATION command is used 3 times 
to input the same dummy model and position it as follows: 
4.  Transformation id 1000 imports the dummy model (dummy.k) and rotates it 45 
degrees about 𝑧-axis at the point (0.0,0.0,0.0).  Transformation id 1001 performs 
the same transformation using the POINT option. 
5.  Transformation  id  2000  imports  the  same  dummy  model  (dummy.k)  and 
translates 1000 units in the 𝑥 direction. 
6.  Transformation  id  3000  imports  the  same  dummy  model  (dummy.k)  and 
translates  2000  units  in  the  x  direction.    For  each  *DEFINE_TRANSFORMA-
TION, the commands TRANSL, SCALE, and ROTATE are available.  The trans-
formations  are  applied  in  the  order  in  which  they  are  defined  in  the  file,  e.g., 
transformation  id  1000  in  this  example  would  translate,  scale  and  then  rotate 
the  model.    *INCLUDE_TRANSFORM  uses  a  transformation  id  defined  by  a 
*DEFINE_TRANSFORMATION command to import a model and perform the 
associated transformations.  It also allows the user upon importing the model to 
apply  offsets  to  the  various  entity  ids  and  perform  unit  conversion  of  the  im-
ported model. 
*KEYWORD 
*DEFINE_TRANSFORMATION 
      1000   
$ option &       dx&       dy&       dz& 
TRANSL        0000.0       0.0       0.0 
$ option &       dx&       dy&       dz& 
SCALE           1.00       1.0       1.0 
$ option &       dx&       dy&       dz&       px&       py&       pz&    
angle& 
ROTATE          0.00       0.0       1.0      0.00      0.00       0.0     
45.00 
*DEFINE_TRANSFORMATION 
      1001 
POINT  
 1       0.0       0.0       0.0 
POINT              2       0.0       0.0       1.0 
ROTATE             1         2      45.0       
*DEFINE_TRANSFORMATION  
      2000 
$ option &       dx&       dy&       dz& 
TRANSL        1000.0       0.0       0.0 
*DEFINE_TRANSFORMATION 
$ tranid & 
     3000 
$ option &       dx&       dy&       dz& 
TRANSL        2000.0       0.0       0.0 
*INCLUDE_TRANSFORM 
dummy.k 
$idnoff  &   ideoff&   idpoff& idmoff  &  idsoff &  iddoff&  iddoff & 
         0         0         0         0         0        0         0 
$  idroff&   ilctmf& 
         0         0 
$  fctmas&   fcttim&   fctlen&  fcttem &   incout& 
    1.0000    1.0000      1.00       1.0         1 
$ tranid & 
      1000 
*INCLUDE_TRANSFORM 
dummy.k 
$idnoff  &   ideoff&   idpoff& idmoff  &  idsoff &  iddoff&  iddoff & 
   1000000   1000000   1000000   1000000   1000000  1000000   1000000 
$  idroff&   ilctmf& 
   1000000   1000000 
$  fctmas&   fcttim&   fctlen&  fcttem &   incout& 
    1.0000    1.0000      1.00       1.0         1 
$ tranid & 
      2000 
*INCLUDE_TRANSFORM 
dummy.k 
$idnoff  &   ideoff&   idpoff& idmoff  &  idsoff &  iddoff&  iddoff & 
   2000000   2000000   2000000   2000000   2000000  2000000   2000000 
$  idroff&   ilctmf& 
   2000000   2000000 
$  fctmas&   fcttim&   fctlen&  fcttem &   incout& 
    1.0000    1.0000      1.00       1.0         1 
$ tranid &
3000 
*END
*DEFINE_TRIM_SEED_POINT_COORDINATES 
Purpose:  The keyword is developed to facilitate blank trimming in a stamping line die 
simulation.  It allows for the trimming process and inputs to be defined independent of 
the previous process simulation results, and is applicable to shell, solid and laminate. 
  Card 1 
1 
Variable 
NSEED 
Type 
I 
Default 
none 
2 
X1 
F 
0 
3 
Y1 
F 
0 
4 
Z1 
F 
0 
5 
X2 
F 
0 
6 
Y2 
F 
7 
Z2 
F 
0.0 
0.0 
8 
  VARIABLE   
DESCRIPTION
NSEED 
Number of seed points.  Maximum value of “2” is allowed. 
X1, Y1, Z1 
Location coordinates of seed point #1. 
X2, Y2, Z2 
Location coordinates of seed point #2. 
Remarks: 
1.  This  keyword  is  used  in  conjunction  with  keywords  *ELEMENT_TRIM  and 
*DEFINE_CURVE_TRIM, where variables NSEED1 and NSEED2 should be left 
as  blank.    For  detailed  usage,  refer  to  Seed  Node  Definition  section  in  *DE-
FINE_CURVE_TRIM. 
2.  Variable NSEED is set to the number of seed points desired.  For example, in a 
double attached drawn panel trimming, NSEED would equal to 2. 
3.  A partial keyword inputs for a single drawn panel trimming is listed below.  
*INCLUDE_TRIM 
drawn.dynain 
*ELEMENT_TRIM 
         1 
*DEFINE_CURVE_TRIM_NEW 
$#    TCID    TCTYPE      TFLG      TDIR     TCTOL      TOLN     NSEED 
         1         2                  11     0.250                     
trimlines.iges 
*DEFINE_TRIM_SEED_POINT_COORDINATES 
$    NSEED        X1       Y1         Z1       X2        Y2        Z2 
         1    -271.4    89.13   1125.679 
*DEFINE_VECTOR 
11,0.0,0.0,0.0,0.0,0.0,10.0
Typically,  seed  point  coordinates  can  be  selected  from  the  stationary  post  in 
punch home position. 
4.  This feature is available in LS-DYNA R4 Revision 53048 and later releases.
*DEFINE_VECTOR 
Purpose:  Define a vector by defining the coordinates of two points. 
Card 
1 
Variable 
VID 
Type 
Default 
I 
0 
Remarks 
2 
XT 
F 
3 
YT 
F 
4 
ZT 
F 
5 
XH 
F 
6 
YH 
F 
7 
ZH 
F 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
8 
CID 
I 
0 
  VARIABLE   
DESCRIPTION
VID 
Vector ID 
X-coordinate of tail of vector 
Y-coordinate of tail of vector 
Z-coordinate of tail of vector 
X-coordinate of head of vector 
Y-coordinate of head of vector 
Z-coordinate of head of vector 
Coordinate system ID to define vector in local coordinate system.
All  coordinates,  XT,  YT,  ZT,  XH,  YH,  and  ZH  are  in  respect  to
CID. 
EQ.0: global (default). 
XT 
YT 
ZT 
XH 
YH 
ZH 
CID 
Remarks: 
1.The coordinates should differ by a certain margin to avoid numerical inaccuracies.
Purpose:  Define a vector with two nodal points. 
*DEFINE 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VID 
NODET 
NODEH 
Type 
Default 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
VID 
Vector ID 
NODET 
Nodal point to define tail of vector 
NODEH 
Nodal point to define head of vector
EXAMPLES 
The following examples demonstrate the input for these options: 
*DEFINE_BOX 
*DEFINE_COORDINATE_NODES, 
*DEFINE_COORDINATE_SYSTEM, 
*DEFINE_COORDINATE_VECTOR 
*DEFINE_CURVE 
*DEFINE_SD_ORIENTATION 
*DEFINE_VECTOR commands. 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *DEFINE_BOX 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Define box number eight which encloses a volume defined by two corner 
$  points: (-20.0, -39.0, 0.0) and (20.0, 39.0, 51.0).  As an example, this 
$  box can be used as an input for the *INITIAL_VELOCITY keyword in which 
$  all nodes within this box are given a specific initial velocity. 
$ 
*DEFINE_BOX 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$    boxid       xmm       xmx       ymn       ymx       zmn       zmx 
         8     -20.0      20.0     -39.0      39.0       0.0      51.0 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *DEFINE_COORDINATE_NODES 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Define local coordinate system number 5 using three nodes: 10, 11 and 20. 
$  Nodes 10 and 11 define the local x-direction.  Nodes 10 and 20 define 
$  the local x-y plane. 
$ 
$  For example, this coordinate system (or any coordinate system defined using 
$  a *DEFINE_COORDINATE_option keyword) can be used to define the local 
$  coordinate system of a joint, which is required in order to define joint 
$  stiffness using the *CONSTRAINED_JOINT_STIFFNESS_GENERALIZED keyword. 
$ 
*DEFINE_COORDINATE_NODES 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      cid        n1        n2        n3 
         5        10        11        20 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *DEFINE_COORDINATE_SYSTEM 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Define local coordinate system number 3 using three points.  The origin of 
$  local coordinate system is at (35.0, 0.0, 0.0).  The x-direction is defined 
$  from the local origin to (35.0, 5.0, 0.0).  The x-y plane is defined using 
$  the vector from the local origin to (20.0, 0.0, 20.0) along with the local 
$  x-direction definition. 
$ 
*DEFINE_COORDINATE_SYSTEM 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      cid        Xo        Yo        Zo        Xl        Yl        Zl 
         3      35.0       0.0       0.0      35.0       5.0       0.0 
$ 
$       Xp        Yp        Zp 
      20.0       0.0      20.0 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *DEFINE_COORDINATE_VECTOR 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Define local coordinate system number 4 using two vectors. 
$    Vector 1 is defined from (0.0, 0.0, 0.0) to (1.0, 1.0, 0.0) 
$    Vector 2 is defined from (0.0, 0.0, 0.0) to (1.0, 1.0, 1.0) 
$  See the corresponding keyword command for a description. 
$ 
*DEFINE_COORDINATE_VECTOR 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      cid        Xx        Yx        Zx        Xv        Yv        Zv 
         4       1.0       1.0       0.0       1.0       1.0       1.0 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *DEFINE_CURVE 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Define curve number 517.  This particular curve is used to define the 
$  force-deflection properties of a spring defined by a *MAT_SPRING_INELASTIC 
$  keyword.  The abscissa value is offset 25.0 as a means of modeling a gap 
$  at the front of the spring.  This type of spring would be a compression 
$  only spring. 
$ 
*DEFINE_CURVE 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$     lcid      sidr      scla      sclo      offa      offo 
       517                                    25.0 
$ 
$           abscissa            ordinate 
                 0.0                 0.0 
                80.0                58.0 
                95.0                35.0 
               150.0                44.5 
               350.0                45.5 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *DEFINE_SD_ORIENTATION 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  A discrete spring is defined with two nodes in 3-D space.  However, it is 
$  desired to have the force of that spring to act only in the z-direction. 
$  The following definition makes this happen.  Additionally, vid = 7 
$  must be specified in the *ELEMENT_DISCRETE keyword for this spring. 
$ 
*DEFINE_SD_ORIENTATION 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      vid       iop        xt        yt        zt      nid1      nid2 
         7         0       0.0       0.0       1.0 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *DEFINE_VECTOR 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Define vector number 5 from (0,0,0) to (0,1,1).  As an example, this vector 
$  can be used to define the direction of the prescribed velocity of a node 
$  using the *BOUNDARY_PRESCRIBED_MOTION_NODE keyword. 
$ 
*DEFINE_VECTOR 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      vid        xt        yt        zt        xh        yh        zh 
         3       0.0       0.0       0.0       0.0       1.0       1.0 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
The cards in this section are defined in alphabetical order and are as follows: 
*DEFORMABLE_TO_RIGID 
*DEFORMABLE_TO_RIGID_AUTOMATIC 
*DEFORMABLE_TO_RIGID_INERTIA 
If one of these cards is defined, then any deformable part defined in the model may be 
switched to rigid during the calculation.  Parts that are defined as rigid (*MAT_RIGID) 
in the input are permanently rigid and cannot be changed to deformable. 
Deformable parts may be switched to rigid at the start of the calculation by specifying 
them on the *DEFORMABLE_TO_RIGID card. 
Part switching may be specified on a restart  or it 
may  be  performed  automatically  by  use  of  the  *DEFORMABLE_TO_RIGID_AUTO-
MATIC cards.   
The *DEFORMABLE_TO_RIGID_INERTIA cards allow inertial properties to be defined 
for deformable parts that are to be swapped to rigid at a later stage. 
It is not possible to perform part material switching on a restart if it was not flagged in 
the  initial  analysis.    The  reason  for  this  is  that  extra  memory  needs  to  be  set  up 
internally  to  allow  the  switching  to  take  place.    If  part  switching  is  to  take  place  on  a 
restart,  but  no  parts  are  to  be  switched  at  the  start  of  the  calculation,  no  inertia 
properties  for  switching  and  no  automatic  switching  sets  are  to  be  defined,  then  just 
define one *DEFORMABLE_TO_RIGID card without further input.
*DEFORMABLE_TO_RIGID 
Purpose:  Define materials to be switched to rigid at the start of the calculation. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
MRB 
PTYPE 
Type 
I 
Default 
none 
A 
I 
0 
  VARIABLE   
DESCRIPTION
PID 
MRB 
Part ID of the part which is switched to a rigid material, also see
*PART. 
Part ID of the master rigid body to which the part is merged.  If
zero,  the  part  becomes  either  an  independent  or  master  rigid
body. 
PTYPE 
Type of PID: 
EQ.“PART”: PID is a part ID. 
EQ.“PSET”:  PID is a part set ID.  All parts included in part set
PID will be switched to rigid at the start of the cal-
culation.
*DEFORMABLE_TO_RIGID_AUTOMATIC 
Purpose:  Define a set of parts to be switched to rigid or to deformable at some stage in 
the calculation  This keyword’s data cards are enumerated below: 
•  2 parameter cards: see “Card 1” and “Card 2” below 
•  D2R  instances of “Card 3” 
•  R2D  instances of “Card 4” 
•  Total number of cards = 2 + D2R + R2D 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SWSET 
CODE 
TIME 1 
TIME 2 
TIME 3 
ENTNO 
RELSW 
PAIRED 
Type 
I 
Default 
none 
Remark 
  Card 2 
1 
I 
0 
1 
2 
F 
0. 
F 
1020 
F 
0. 
I 
0 
I 
0. 
1, 2 
3 
4 
5 
6 
7 
I 
0 
3 
8 
Variable 
NRBF 
NCSF 
RWF 
DTMAX 
D2R 
R2D 
OFFSET 
Type 
Default 
I 
0 
I 
0 
I 
0 
F 
0. 
I 
0 
I 
0 
F 
0 
  VARIABLE   
DESCRIPTION
SWSET 
Set number for this automatic switch set.  Must be unique. 
CODE 
Activation switch code.  Defines the test to activate the automatic
material switch of the part: 
EQ.0: switch takes place at time 1, 
EQ.1: switch takes place between time 1 and time 2 if rigid wall
force (specified below) is zero, 
EQ.2: switch  takes  place  between  time  1  and  time  2  if  contact
VARIABLE   
DESCRIPTION
surface force (specified below) is zero, 
EQ.3: switch takes place between time 1 and time 2 if rigid wall
force (specified below) is non-zero, 
EQ.4: switch  takes  place  between  time  1  and  time  2  if  contact
surface force (specified below) is non-zero. 
EQ.5:  switch 
is  controlled  by  *SENSOR_CONTROL  with 
  When 
column  8,
TYPE = DEF2RIG,  see  *SENSOR_CONTROL. 
CODE = 5, 
TIME1~PAIRED, are ignored. 
column  3 
inputs  of 
to 
TIME1 
TIME2 
TIME3 
Switch will not take place before this time. 
Switch will not take place after this time: 
EQ.0:  Time 2 set to 1020 
Delay  period.    After  this  part  switch  has  taken  place,  another
automatic switch will not take place for the duration of the delay
period.    If  set  to  zero  a  part  switch  may  take  place  immediately 
after this switch. 
ENTNO 
Rigid wall/contact surface number for switch codes 1, 2, 3, 4. 
RELSW 
Related  switch  set.    The  related  switch  set  is  another  automatic
switch set that must be activated before this part switch can take
place: 
EQ.0: no related switch set. 
PAIRED 
Define a pair of related switches. 
EQ.0:  not paired 
EQ.1:  paired with switch set RELSW and is the Master switch.
EQ.-1: paired with switch set RELSW and is the Slave switch.
VARIABLE   
NRBF 
DESCRIPTION
Nodal rigid body flag. 
For  all  values  of  NRBF,  nodal  rigid  bodies  defined  using  *CON-
STRAINED_NODAL_RIGID_BODY and *CONSTRAINED_GEN-
ERALIZED_WELD_OPTION, which share any nodes with a rigid 
body  created  by  deformable-to-rigid  switching,  are  merged  with 
the  latter  to  form  a  single  rigid  body.    Other  actions  dependent 
upon the value of NRBF are: 
EQ.0: no further action, 
EQ.1: delete  all  remaining  nodal  rigid  bodies,  that  is,  delete
those  nodal  rigid  bodies  that  do  not  share  any  nodes
with a rigid body created by deformable-to-rigid switch-
ing, 
EQ.2: Activate nodal rigid bodies. 
NCSF 
Nodal constraint set flag. 
If  nodal  constraint/spot  weld  definitions  are  active  in  the
deformable bodies that are switched to rigid, then the definitions
should be deleted to avoid instabilities: 
EQ.0: no change, 
EQ.1: delete, 
EQ.2: activate. 
RWF 
Flag to delete or activate rigid walls: 
EQ.0: no change, 
EQ.1: delete, 
EQ.2: activate. 
DTMAX 
Maximum permitted time step size after switch. 
D2R 
Number of deformable parts to be switched to rigid plus number
of  rigid  parts 
for  which  new  master/slave  rigid  body
combinations will be defined: 
EQ.0: no parts defined. 
R2D 
Number of rigid parts to be switched to deformable: 
EQ.0: no parts defined.
VARIABLE   
OFFSET 
DESCRIPTION
Optional contact thickness for switch to deformable.  For contact, 
its  value  should  be  set  to  a  value  greater  than  the  contact
thickness  offsets  to  ensure  the  switching  occurs  prior  to  impact.
This  option  applies  if  and  only  if  CODE  is  set  to  3  or  4.    For
CODE = 3 all rigid wall options are implemented.  For CODE = 4, 
the  implementation  works  for  the  contact  type  CONTACT_AU-
TOMATIC_when  the  options:  ONE_WAY_SURFACE_TO_SUR-
FACE,    NODES_TO_SURFACE,  and  SUR-FACE_TO_SURFACE 
are invoked.   
Deformable to Rigid Cards.  D2R additional cards with one for each part. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
MRB 
PTYPE 
Type 
I 
Default 
none 
A 
I 
0 
  VARIABLE   
DESCRIPTION
PID 
MRB 
Part  ID  of  the  part  which  is  switched  to  a  rigid  material.    When
PID is merged to another rigid body by the MRB field, this part is
allowed to be rigid before the switch. 
Part ID of the master rigid body to which part PID is merged.  If
zero,  part  PID  becomes  either  an  independent  or  master  rigid
body. 
PTYPE 
Type of PID:  
EQ.“PART”: PID is a part ID. 
EQ.“PSET”:  PID is a part set ID.
Rigid to Deformable Cards.  R2D additional cards with one for each part. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
PTYPE 
Type 
I 
A 
Default 
none 
  VARIABLE   
DESCRIPTION
PID 
Part ID of the part which is switched to a deformable material. 
PTYPE 
Type of PID:  
EQ.“PART”: PID is a part ID. 
EQ.“PSET”:  PID is a part set ID. 
Remarks: 
1.  Allowed Contact Types.  Only surface to surface and node to surface contacts 
can be used to activate an automatic part switch. 
2.  Rigid  Wall  Numbering.    Rigid  wall  numbers  are  the  order  in  which  they  are 
defined  in  the  deck.    The  first  rigid  wall  and  the  first  contact  surface  encoun-
tered in the input deck will have an entity number of 1.  The contact surface id 
is that as defined on the *CONTACT_…_ID card. 
3.  Paired  Switches.    Switch  sets  may  be  paired  together  to  allow  a  pair  of 
switches  to  be  activated  more  than  once.    Each  pair  of  switches  should  use 
consistent values for CODE, i.e.  1 & 3 or 2 & 4.  Within each pair of switches, 
the  related  switch,  RELSW,  should  be  set  to  the  ID  of  the  other  switch  in  the 
pair.  The Master switch (PAIRED = 1) will be activated before the Slave switch 
(PAIRED = -1).  Pairing allows the multiple switches to take place as for exam-
ple when contact is made and lost several times during an analysis. 
If the delete switch is activated, ALL corresponding constraints are deactivated 
regardless of their relationship to a switched part.  By default, constraints which 
are directly associated with a switched part are deactivated/activated as neces-
sary. 
$  Define a pair or related switches that will be activated by (no)force on  
$  Contact 3.  To start with switch set 20 will be activated (PAIRED=1) 
swapping
$  the PARTS to RIGID.  When the contact force is none zero switch set 10 will 
be  
$  activated swapping the PARTS to DEFORMABLE.  If the contact force returns 
to  
$  zero switch set 20 will be activated again making the PARTS RIGID. 
$ 
*DEFORMABLE_TO_RIGID_AUTOMATIC 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>...
.8 
$    swset      code    time 1    time 2    time 3     entno     relsw    
paired 
        20         2                                       3        10         
1 
$     nrbf      ncsf       rwf     dtmax       D2R       R2D 
                                                 1 
*DEFORMABLE_TO_RIGID_AUTOMATIC 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>...
.8 
$    swset      code    time 1    time 2    time 3     entno     relsw    
paired 
        10         4                                       3        20        
-1 
$     nrbf      ncsf       rwf     dtmax       D2R       R2D 
                                                    1
*DEFORMABLE_TO_RIGID_INERTIA 
Purpose:    Inertial  properties  can  be  defined  for  the  new  rigid  bodies  that  are  created 
when the deformable parts are switched.  These can only be defined in the initial input 
if they are needed in a later restart.  Unless these properties are defined, LS-DYNA will 
recompute  the  new  rigid  body  properties  from  the  finite  element  mesh.    The  latter 
requires  an  accurate  mesh  description.    When  rigid  bodies  are  merged  to  a  master 
rigid  body,  the  inertial  properties  defined  for  the  master  rigid  body  apply  to  all 
members of the merged set. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
Type 
I 
Default 
none 
  Card 2 
Variable 
1 
XC 
Type 
F 
  Card 3 
1 
Variable 
IXX 
2 
YC 
F 
2 
IXY 
3 
ZC 
F 
3 
IXZ 
4 
TM 
F 
4 
IYY 
5 
6 
7 
8 
5 
IYZ 
6 
IZZ 
7 
8 
Type 
F 
F 
F 
F 
F 
F 
Default 
none 
0.0 
0.0 
none 
0.0 
none 
  VARIABLE   
DESCRIPTION
PID 
XC 
YC 
Part ID, see *PART. 
x-coordinate of center of mass 
y-coordinate of center of mass
VARIABLE   
DESCRIPTION
ZC 
TM 
IXX 
IXY 
IXZ 
IYY 
IYZ 
IZZ 
z-coordinate of center of mass 
Translational mass 
Ixx (the xx component of inertia tensor) 
Ixy 
Ixz 
Iyy 
Iyz 
Izz
The element cards in this section are defined in alphabetical order: 
*ELEMENT_BLANKING 
*ELEMENT_BEAM_{OPTION}_{OPTION} 
*ELEMENT_BEAM_PULLEY 
*ELEMENT_BEAM_SOURCE 
*ELEMENT_DIRECT_MATRIX_INPUT 
*ELEMENT_DISCRETE_{OPTION} 
*ELEMENT_DISCRETE_SPHERE_{OPTION} 
*ELEMENT_GENERALIZED_SHELL 
*ELEMENT_GENERALIZED_SOLID 
*ELEMENT_INERTIA_{OPTION} 
*ELEMENT_INTERPOLATION_SHELL 
*ELEMENT_INTERPOLATION_SOLID 
*ELEMENT_LANCING 
*ELEMENT_MASS_{OPTION} 
*ELEMENT_MASS_MATRIX_{OPTION} 
*ELEMENT_MASS_PART_{OPTION} 
*ELEMENT_PLOTEL 
*ELEMENT_SEATBELT 
*ELEMENT_SEATBELT_ACCELEROMETER 
*ELEMENT_SEATBELT_PRETENSIONER 
*ELEMENT_SEATBELT_RETRACTOR 
*ELEMENT_SEATBELT_SENSOR
*ELEMENT_SHELL_{OPTION} 
*ELEMENT_SHELL_NURBS_PATCH 
*ELEMENT_SHELL_SOURCE_SINK 
*ELEMENT_SOLID_{OPTION} 
*ELEMENT_SOLID_NURBS_PATCH 
*ELEMENT_SPH 
*ELEMENT_TRIM 
*ELEMENT_TSHELL_{OPTION} 
The ordering of the element cards in the input file is completely arbitrary.  An arbitrary 
number of element blocks can be defined preceded by a keyword control card.
*ELEMENT 
Purpose:  This keyword is used to define a part set to be used in keyword *DEFINE_-
FORMING_BLANKMESH for a blank mesh generation. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PSID 
Type 
I 
Default 
none 
  VARIABLE   
DESCRIPTION
PSID 
Part set ID, defined by *SET_PART. 
Remarks: 
1.  This keyword is used in conjunction with *DEFINE_FORMING_BLANKMESH 
to generate mesh on a sheet blank for metal forming simulation. 
2.  This feature is available in LS-DYNA R5 Revision 59165 or later releases.
*ELEMENT_BEAM_{OPTION}_{OPTION} 
Available options include: 
<BLANK> 
THICKNESS, SCALAR, SCALR or SECTION 
PID 
OFFSET 
ORIENTATION 
WARPAGE 
ELBOW (beta) 
Purpose:    Define  two  node  elements  including  3D  beams,  trusses,  2D  axisymmetric 
shells, and 2D plane strain beam elements.  The type of the element and its formulation 
is specified through the part ID  and the section ID .   
Two  alternative  methods  are  available  for  defining  the  cross  sectional  property  data.  
The THICKNESS and SECTION options are provided for the user to override the *SEC-
TION_BEAM data which is taken as the default if the THICKNESS or SECTION option 
is not used.  . The SECTION option applies only to resultant beams (ELFORM.eq.2 on 
*SECTION_BEAM).    End  release  conditions  are  imposed  using  constraint  equations, 
and  caution  must  be  used  with  this  option  as  discussed  in  remark  2  below.    The 
SCALAR/SCALR options applies only to material model type 146, *MAT_1DOF_GEN-
ERALIZED_SPRING. 
The PID option is used by the type 9 spot weld element only and is ignored for all other 
beam  types.    When  the  PID  option  is  active  an  additional  card  is  read  that  gives  two 
part ID's that are tied by the spot weld element.  If the PID option is inactive for the type 
9  element  the  nodal  points  of  the  spot  weld  are  located  to  the  two  nearest  master 
segments.  In either case, *CONTACT_SPOTWELD must be defined with the spot weld 
beam part as slave and the shell parts (including parts PID1 and PID2) as master.  The 
surface  of  each  segment  should  project  to  the  other  and  in  the  most  typical  case  the 
node  defining  the  weld,  assuming  only  one  node  is  used,  should  lie  in  the  middle; 
however,  this  is  not  a  requirement.    Note  that  with  the  spot  weld  elements  only  one 
node is needed to define the weld, and two nodes are optional. 
The options ORIENTATION and OFFSET are not available for discrete beam elements.   
The  ELBOW  option  is  a  3-node  beam  element  with  quadratic  interpolation  that  is 
tailored  for  the  piping  industry.    It  includes  12  degrees  of  freedom,  including  6 
ovalization degrees of freedom for describing the ovalization, per node.  That is a total
of 36 DOFs for each element.  An internal pressure can also be given that tries to stiffen 
the pipe.  The pressure, if activated accordingly, can also contribute to the elongation of 
the pipe.  The control node must be given but it is only used for initially straight elbow 
elements.    For  curved  elements  the  curvature  center  is  used  as  the  control  node.    See 
*SECTION_BEAM for more information about the physical properties such as pressure 
and output options.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
EID 
PID 
N1 
N2 
N3 
RT1 
RR1 
RT2 
RR2 
LOCAL
Type 
I 
I 
I 
I 
I 
I 
Default 
none  none  none  none  none 
0 
I 
0 
I 
0 
I 
0 
I 
2 
Remarks 
1 
2,3 
2,3 
2,3 
2,3 
2,3 
Thickness Card.  Additional Card for THICKNESS keyword option.  
Card 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
PARM1 
PARM2 
PARM3 
PARM4 
PARM5 
Type 
Remarks 
F 
5 
F 
5 
F 
5 
F 
5 
Section Card.  Additional card required for SECTION keyword option. 
Card 
1 
Variable 
STYPE 
Type 
A 
2 
D1 
F 
3 
D2 
F 
4 
D3 
F 
5 
D4 
F 
6 
D5 
F 
7 
D6 
F 
F 
5,6 
8 
Remarks
Scalar card.  Additional card for SCALAR keyword option. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
VOL 
INER 
Type 
F 
F 
CID 
F 
DOFN1 
DOFN2 
F 
F 
Scalar Card (alternative).  Additional card for SCALR keyword option.  
Card 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
VOL 
INER 
CID1 
CID2 
DOFNS 
Type 
F 
F 
F 
F 
F 
Spot Weld Part Card.  Additional card for PID keyword option. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
PID1 
PID2 
Type 
I 
I 
Default 
none  none 
Remarks
Offset Card.  Additional card for OFFSET keyword option. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
WX1 
WY1 
WZ1 
WX2 
WY2 
WZ2 
Type 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Remarks 
8 
8 
8 
8 
8 
8 
Orientation Card.  Additional card for ORIENTATION keyword option.  
4 
5 
6 
7 
8 
Card 
Variable 
1 
VX 
Type 
F 
2 
VY 
F 
3 
VZ 
F 
Default 
0.0 
0.0 
0.0 
Remarks 
Warpage Card.  Additional card for WARPAGE keyword option. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SN1 
SN2 
Type 
I 
I 
Default 
none 
none 
Remarks
Elbow Card.  Additional card for ELBOW keyword option. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MN 
Type 
I 
Default 
none 
Remarks 
  VARIABLE   
EID 
PID 
N1 
N2 
N3 
DESCRIPTION
Element ID.  A unique ID is generally required, i.e., EID must be
different from the element ID’s also defined under *ELEMENT_-
DISCRETE  and  *ELEMENT_SEATBELT.      If  the  parameter, 
BEAM,  is set to 1 on the keyword input for *DATABASE_BINA-
RY_D3PLOT,    the  null  beams  used  for  visualization  are  not
created for the latter two types, and the ID’s used for the discrete
elements  and  the  seatbelt  elements  can  be  identical  to  those
defined here. 
Part ID, see *PART. 
Nodal point (end) 1. 
Nodal  point  (end)  2.    This  node  is  optional  for  the  spot  weld,
beam type 9, since if it not defined it will be created automatically
and given a non-conflicting nodal point ID.  Nodes N1 and N2 are 
automatically positioned for the spot weld beam element.  For the
zero length discrete beam elements where one end is attached to
ground, set N2 = -N1.  In this case, a fully constrained nodal point 
will be created with a unique ID for node N2. 
Nodal point 3 for orientation.  The third node, N3, is optional for
beam  types  3,  6,  7,  8,  and  if  the  cross-section    is  circular,  beam 
types 1 and 9.  The third node is used for the discrete beam, type
6,  if  and  only  if  SCOOR  is  set  to  2.0  in  the  *SECTION_BEAM 
input,  but  even  in  this  case  it  is  optional.    An  orientation  vector
can  be  defined  directly  by  using  the  option,  ORIENTATION.    In 
this case N3 can be defined as zero. 
RT1, RT2 
Release  conditions  for  translations  at  nodes  N1  and  N2,
VARIABLE   
DESCRIPTION
respectively: 
EQ.0: no translational degrees-of-freedom are released 
EQ.1: x-translational degree-of-freedom 
EQ.2: y-translational degree-of-freedom 
EQ.3: z-translational degree-of-freedom 
EQ.4: x and y-translational degrees-of-freedom 
EQ.5: y and z-translational degrees-of-freedom 
EQ.6: z and x-translational degrees-of-freedom 
EQ.7: x, y, and z-translational degrees-of-freedom (3DOF) 
This option does not apply to the spot weld, beam type 9. 
RR1, RR2 
Release conditions for rotations at nodes N1 and N2, respectively:
EQ.0: no rotational degrees-of-freedom are released 
EQ.1: x-rotational degree-of-freedom 
EQ.2: y-rotational degree-of-freedom 
EQ.3: z-rotational degree-of-freedom 
EQ.4: x and y-rotational degrees-of-freedom 
EQ.5: y and z-rotational degrees-of-freedom 
EQ.6: z and x-rotational degrees-of-freedom 
EQ.7: x, y, and z-rotational degrees-of-freedom (3DOF) 
This option does not apply to the spot weld, beam type 9. 
LOCAL 
Coordinate system option for release conditions: 
EQ.1: global coordinate system 
EQ.2: local coordinate system (default) 
PARM1 
Based on beam type: 
Type.EQ.1:  beam thickness, s direction at node 1 
Type.EQ.2:  area 
Type.EQ.3:  area 
Type.EQ.4:  beam thickness, s direction at node 1 
Type.EQ.5:  beam thickness, s direction at node 1
VARIABLE   
DESCRIPTION
Type.EQ.6: volume, see description for VOL below. 
Type.EQ.7:  beam thickness, s direction at node 1 
Type.EQ.8:  beam thickness, s direction at node 1 
Type.EQ.9:  beam thickness, s direction at node 1 
PARM2 
Based on beam type: 
Type.EQ.1:  beam thickness, s direction at node 2 
Type.EQ.2:  Iss 
Type.EQ.3:  ramp-up time for dynamic relaxation 
Type.EQ.4:  beam thickness, s direction at node 2 
Type.EQ.5:  beam thickness, s direction at node 2 
Type.EQ.6:  Inertia, see description for INER below. 
Type.EQ.7:  beam thickness, s direction at node 2 
Type.EQ.8:  beam thickness, s direction at node 2 
Type.EQ.9:  beam thickness, s direction at node 2 
PARM3 
Based on beam type: 
Type.EQ.1:  beam thickness, t direction at node 1 
Type.EQ.2:  Itt 
Type.EQ.3:  initial stress for dynamic relaxation 
Type.EQ.4:  beam thickness, t direction at node 1 
Type.EQ.5:  beam thickness, t direction at node 1 
Type.EQ.6:  local coordinate ID 
Type.EQ.7:  not used. 
Type.EQ.8:  not used. 
Type.EQ.9:  beam thickness, t direction at node 1 
PARM4 
Based on beam type: 
Type.EQ.1:  beam thickness, t direction at node 2 
Type.EQ.2:  Irr 
Type.EQ.3:  not used 
Type.EQ.4:  beam thickness, t direction at node 2
VARIABLE   
DESCRIPTION
Type.EQ.5: beam thickness, t direction at node 2 
Type.EQ.6:  area 
Type.EQ.7:  not used. 
Type.EQ.8:  not used. 
Type.EQ.9:  beam thickness, t direction at node 2 
PARM5 
Based on beam type: 
Type.EQ.1:  not used 
Type.EQ.2:  shear area 
Type.EQ.3:  not used 
Type.EQ.4:  not used 
Type.EQ.5:  not used 
Type.EQ.6:  offset 
Type.EQ.7:  not used. 
Type.EQ.8:  not used. 
Type.EQ.9:  print  flag  to  SWFORC  file.    The  default  is  taken
from  the  SECTION_BEAM  input.    To  override  set 
PARM5  to  1.0  to  suppress  printing,  and  to  2.0  to
print. 
STYPE 
Section type (A format) of resultant beam, see Figure 36-1: 
EQ.SECTION_01: I-Shape 
EQ.SECTION_02: Channel 
EQ.SECTION_03: L-Shape 
EQ.SECTION_04: T-Shape 
EQ.SECTION_05: Tubular box 
EQ.SECTION_06:Z-Sape 
EQ.SECTION_07: Trapezoidal 
EQ.SECTION_08: Circular 
EQ.SECTION_09: Tubular 
EQ.SECTION_10: I-Shape 2 
EQ.SECTION_11: Solid box 
EQ.SECTION_12: Cross 
EQ.SECTION_13: H-Shape 
EQ.SECTION_14: T-Shape 2 
EQ.SECTION_15: I-Shape 3 
EQ.SECTION_16: Channel 2 
EQ.SECTION_17: Channel 3 
EQ.SECTION_18: T-Shape 3 
EQ.SECTION_19: Box-Shape 2
EQ.SECTION_20: Hexagon 
EQ.SECTION_21: Hat-Shape 
EQ.SECTION_22: Hat-Shape 2 
D1-D6 
Input parameters for section option using STYPE above.
VARIABLE   
DESCRIPTION
PID1 
PID2 
VOL 
INER 
CID 
DOFN1 
DOFN2 
CID1 
CID2 
Optional part ID for spot weld element type 9. 
Optional part ID for spot weld element type 9. 
Volume of discrete beam and scalar (MAT_146) beam.  If the mass 
density of the material model for the discrete beam is set to unity,
the  magnitude  of  the  lumped  mass  can  be  defined  here  instead.
This  lumped  mass  is  partitioned  to  the  two  nodes  of  the  beam 
element.    The  translational  time  step  size  for  the  type  6  beam  is
dependent  on  the  volume,  mass  density,  and  the  translational
stiffness  values,  so  it  is  important  to  define  this  parameter.
Defining the volume is also essential for mass scaling if the type 6 
beam controls the time step size. 
Mass  moment  of  inertia  for  the  six  degree  of  freedom  discrete
beam  and  scalar  (MAT_146)  beam.    This  lumped  inertia  is 
partitioned to the two nodes of the beam element.  The rotational
time  step  size  for  the  type  6  beam  is  dependent  on  the  lumped 
inertia  and  the  rotational  stiffness  values,  so  it  is  important  to
define this parameter if the rotational springs are active.  Defining
the rotational inertia is also essential for mass scaling if the type 6
beam rotational stiffness controls the time step size. 
Coordinate system ID for orientation, material type 146, see *DE-
FINE_COORDINATE_SYSTEM.    If  CID = 0,  a  default  coordinate 
system is defined in the global system. 
Active  degree-of-freedom  at  node  1,  a  number  between  1  to  6
where  1,  2,  and  3  are  the  x,  y,  and  z-translations  and  4,  5,  and  6 
are  the  x,  y,  and  z-rotations.    This  degree-of-freedom  acts  in  the 
local system given by CID above.  This input applies to material 
model type 146. 
Active  degree-of-freedom  at  node  2,  a  number  between  1  to  6.
This  degree-of-freedom  acts  in  the  local  system  given  by  CID
above.  This input applies to material model type 146. 
Coordinate system ID at node 1 for orientation, material type 146, 
see  *DEFINE_COORDINATE_SYSTEM.    If  CID1 = 0,  a  default 
coordinate system is defined in the global system. 
Coordinate system ID at node 2 for orientation, material type 146,
see  *DEFINE_COORDINATE_SYSTEM.    If  CID2 = 0,  a  default 
coordinate system is defined in the global system.
VARIABLE   
DOFNS 
DESCRIPTION
Active  degrees-of-freedom  at  node  1  and  node  2.    A  two-digit 
number,  the  first  for  node  1  and the  second  for  node  2,  between
11  to  66  is  expected    where  1,  2,  and  3  are  the  x,  y,  and  z-
translations  and  4,  5,  and  6  are  the  x,  y,  and  z-rotations.    These 
degrees-of-freedom  acts  in  the  local  system  given  by  CID1  and
CID2  above.    This  input  applies  to  material  model  type  146.    If
DOFNS = 12 the node one has an x-translation and node 2 has a y
translation. 
WX1-WZ1 
Offset vector at nodal point N1.  See Remark 8. 
WX2-WZ2 
Offset vector at nodal point N2.  See Remark 8. 
VX,VY,VZ 
Coordinates of an orientation vector relative to node N1.  In this
case,  the  orientation  vector  points  to  a  virtual  third  node  and  so
the input variable N3 should be left undefined.  
SN1 
SN2 
Scalar  nodal  point  (end)  1.    This  node  is  required  for  the
WARPAGE  option. 
Scalar  nodal  point  (end)  2.    This  node  is  required  for  the 
WARPAGE option.
The third node, i.e. the reference node,
must be unique to each beam element if
the coordinate update option is used,
see *CONTROL_OUTPUT.
n3
n2
n1
Figure  17-1.    LS-DYNA  beam  elements.    Node  n3  determines  the  initial 
orientation of the cross section. 
  VARIABLE   
DESCRIPTION
MN 
Middle node for the ELBOW element.  See Remark 9. 
Remarks: 
1.  A  plane  through  N1,  N2,  and  N3  defines  the  orientation  of  the  principal  r-s 
plane of the beam, see Figure 17-1. 
2.  This  option  applies  to  all  three-dimensional  beam  elements.    The  released 
degrees-of-freedom  can  be  either  global,  or  local  relative to  the  local  beam  co-
ordinate  system,  see  Figure  17-1.    A  local  coordinate  system  is  stored  for  each 
node  of  the  beam  element  and  the  orientation  of  the  local  coordinate  systems 
rotates with the node.  To properly track the response, the nodal points with a 
released resultant are automatically replaced with new nodes to accommodate
the  added  degrees-of-freedom.    Then  constraint  equations  are  used  to  join  the 
nodal points together with the proper release conditions imposed. 
Nodal points which belong to beam elements which have re-
lease  conditions  applied  cannot  be  subjected  to  other  con-
straints  such  as  applied  displacement/velocity/acceleration 
boundary  conditions,  nodal  rigid  bodies,  nodal  constraint 
sets, or any of the constraint type contact definitions. 
Force  type  loading  conditions  and  penalty  based  contact  algorithms  may  be 
used with this option. 
3.  Please  note  that  this  option  may  lead  to  nonphysical  constraints  if  the 
translational degrees-of-freedom are released, but this should not be a problem 
if the displacements are infinitesimal. 
4. 
5. 
If  the  THICKNESS  option  is  not  used,  or  if  THICKNESS  is  used  but  essential 
PARMx values are not provided, beam properties are taken from *SECTION_-
BEAM.   
In  the  case  of  the  THICKNESS  option  for  type  6,  i.e.,  discrete  beam  elements, 
PARM1  through  PARM5  replace  the  first  five  parameters  on  card  2  of  *SEC-
TION_BEAM.    Cables  are  a  subset  of  type  6  beams.    PARM1  is  for  non-cable 
discrete  beams  and  is  optional  for  cables,  PARM2  and  PARM3  apply  only  to 
non-cable discrete beams, and PARM4 and PARM5 apply only to cables. 
6. 
In  the  THICKNESS  option,  PARM5  applies  only  to  beam  types  2,    6  (cables 
only), and 9. 
7.  The stress resultants are output in local coordinate system for the beam.  Stress 
information is optional and is also output in the local system for the beam. 
8.  Beam  offsets  are  sometimes  necessary  for  correctly  modeling  beams  that  act 
compositely with other elements such as shells or other beams.  When the OFF-
SET option is specified, global X, Y, and Z components of two offset vectors are 
given,  one  vector  for  each  of  the  two  beam  nodes.    The  offset  vector  extends 
from  the  beam  node  (N1  or  N2)  to  the  reference  axis  of  the  beam.    The  beam 
reference axis lies at the origin of the local s and t axes.  For beam formulations 
1  and  11,  this  origin  is  halfway  between  the  outermost  surfaces  of  the  beam 
cross-section.  Note that for cross-sections that are not doubly symmetric, e.g, a 
T-section,  the  reference  axis  does  not  pass  through  the  centroid  of  the  cross-
section.      For  beam  formulation  2,  the  origin  is  at  the  centroid  of  the  cross-
section.
n1
n3
n4
n2
Figure  17-2.    LS-DYNA  Elbow  element.    Node  n4  is  the  control  node  and  is
given as the beam center of curvature. 
9.  The  Elbow  beam  is  defined  with  4  nodes,  see  Figure  17-2.    Node n1,  n2  being 
the  end  nodes,  and  node  n3  is  the  middle  node.    It  is  custom  to  set  n3  at  the 
midpoint  of  the  beam.    Node  n4  is  an  orientation  node  that  should  be  at  the 
curvature center of the beam.  If a straight beam is defined initially, the orienta-
tion node must be defined and should be on the convex side of the beam.  If a 
curved beam is defined initially the orientation node is automatically calculated 
as  the  center  of  the  beam  curvature.    However,  an  orientation  node  is  still  re-
quired at the input. 
The  extra  nodes  that  include  the  ovalization  degree  of  freedom  are  written  to 
the messag file during initialization.  These extra nodes have 3 dofs each.  That 
means that there are 2 extra nodes for each physical node.  For example it can 
look something like this: 
ELBOW BEAM:           1 
n1-n3-n2:             1     3     2 
ovalization nodes:    5     7     6 
                      8    10     9 
And  it  means  that  node  1  have  the  ovalization  extra  nodes  5  and  8.    The  first 
line  of  ovalization  nodes  includes  the  c1,  c2  and  c3  parameters,  and  the  second 
line includes the d1, d2 and d3 parameters.  That means that node 5 include c1, c2 
and c3, and node 8 include d1, d2 and d3 for beam node 1.  All ovalization dofs 
can be written to the ascii file “elbwov” if the correct print flag is set on *SEC-
TION_BEAM.  These extra nodes can be constrained as usual nodes.  For exam-
ple for a cantilever beam that is mounted at node 1, the nodes 1, 5 and 8 should 
be  constrained.    The  ovalization  is  approximated  with  the  following  trigono-
metric function:  
𝑤(𝑟, 𝜃) = ∑ ∑ ℎ𝑘(𝑟)(𝑐𝑚
𝑘=1
𝑚=1
𝑘 cos 2𝑚𝜃 + 𝑑𝑚
𝑘 sin 2𝑚𝜃),
−1 ≤ 𝑟 ≤ 1, 0 ≤ 𝜃 < 2𝜋
where hk is the interpolation function at the  physical node k. 
The Elbow beam only supports tubular cross sections and the pipe outer radius, 
a, should be smaller than the pipe bend radius, R.  That is a/R<<1.  Moreover, 
the  ELBOW  beams  have  4  stresses:  axial  rr-,  shear  rs-,  shear  rt-  and  loop-
stresses.  The loop stress is written at each integration point and can be visual-
ized  in  LS-PrePost  with  the  user  fringe  plot  file    “elbwlp.k”.    NOTE  that  the 
loop-stress  is  not  written  to  d3plot  as  default!  The  NEIPB  flag  on  *DATA-
BASE_EXTENT_BINARY  must be set to enable d3plot support. 
Right now there is only basic support from the material library.  The following 
materials  are  currently  supported  for  the  ELBOW  beam  (if  requested  more 
materials might be added in the future):  
*MAT_ELASTIC (MAT_001) 
*MAT_PLASTIC_KINEMATIC (MAT_003) 
*MAT_ELASTIC_PLASTIC_THERMAL (MAT_004) 
*MAT_VISCOELASTIC (MAT_006) 
*MAT_PIECEWISE_LINEAR_PLASTICITY (MAT_024)  
*MAT_DAMAGE_3 (MAT_153, explicit only) 
*MAT_CONCRETE_BEAM (MAT_195)
*ELEMENT_BEAM_PULLEY 
Purpose:  Define pulley for beam elements.  This feature is implemented for truss beam 
elements (*SECTION_BEAM, ELFORM = 3) using materials *MAT_001 and *MAT_156, 
or discrete beam elements (ELFORM = 6) using *MAT_CABLE_DISCRETE_BEAM. 
  Card 1 
1 
2 
3 
4 
Variable 
PUID 
BID1 
BID2 
PNID 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
5 
FD 
F 
6 
FS 
F 
7 
LMIN 
F 
8 
DC 
F 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
PUID 
BID1 
BID2 
PNID 
FD 
FS 
Pulley ID.  A unique number has to be used. 
Truss beam element 1 ID. 
Truss beam element 2 ID. 
Pulley node, NID. 
Coulomb dynamic friction coefficient. 
Optional Coulomb static friction coefficient. 
LMIN 
Minimum length, see notes below. 
DC 
Optional  decay  constant  to  allow  smooth  transition  between  the
static and dynamic friction coefficient, i.e., 
𝜇𝑐 = FD + (FS − FD)𝑒−DC×∣𝑣rel∣ 
Remarks: 
Remarks: 
Elements  1  and  2  should  share  a  node  which  is  coincident  with  the  pulley  node.    The 
pulley node should not be on any beam elements.
Pulleys  allow  continuous  sliding  of  a  truss  beam  element  through  a  sharp  change  of 
angle.    Two  elements  (1  &  2  in  Figure  17-21  of  *ELEMENT_SEATBELT_SLIPRING) 
meet at the pulley.  Node 𝐵 in the beam material remains attached to the pulley node, 
but  beam  material  (in  the  form  of  unstretched  length)  is  passed  from  element  1  to 
element  2  to  achieve  slip.    The amount  of  slip  at  each  time  step  is  calculated  from  the 
ratio  of  forces  in  elements  1  and  2.    The  ratio  of  forces  is  determined  by  the  relative 
angle between elements 1 and 2 and the  coefficient of friction, FD.  The tension in the 
beams are taken as 𝑇1 and 𝑇2, where 𝑇2 is on the high tension side and 𝑇1 is the force on 
the low tension side.  Thus, if 𝑇2 is sufficiently close to 𝑇1, no slip occurs; otherwise, slip 
is just sufficient to reduce the ratio 𝑇2/𝑇1 to 𝑒FC×𝜃, where 𝜃 is the wrap angle, see Figures 
17-22  of  *ELEMENT_SEATBELT_SLIPRING.    The  out-of-balance  force  at  node  𝐵  is 
reacted on the pulley node; the motion of node 𝐵 follows that of pulley node. 
If,  due  to  slip  through  the  pulley,  the  unstretched  length  of  an  element  becomes  less 
than  the  minimum  length  LMIN,  the  beam  is  remeshed  locally:    the  short  element 
passes through the pulley and reappears on the other side .  The new 
unstretched length of 𝑒1 is 1.1 × minimum length.  The force and strain in 𝑒2 and 𝑒3 are 
unchanged;  while  the  force  and  strain  in 𝑒1  are  now  equal  to  those  in  𝑒2.    Subsequent 
slip  will  pass  material  from  𝑒3  to  𝑒1.    This  process  can  continue  with  several  elements 
passing in turn through the pulley. 
To define a pulley, the user identifies the two beam elements which meet at the pulley, 
the friction coefficient, and the pulley node.  If BID1 and BID2 are defined as 0 (zero), 
adjacent  beam  elements  are  automatically  detected.    The  two  elements  must  have  a 
common node coincident with the pulley node.  No attempt should be made to restrain 
or  constrain  the  common  node  for  its  motion  will  automatically  be  constrained  to 
follow the pulley node.  Typically, the pulley node is part of a structure and, therefore, 
beam elements should not be connected to this node directly, but any other feature can 
be attached, including rigid bodies. 
*DATABASE_PLLYOUT can be used to write a time history output database pllyout for 
the pulley which records beam IDs, slip, slip rate, resultant force, and wrap angle.
*ELEMENT_BEAM_SOURCE 
Purpose:    Define  a  nodal  source  for  beam  elements.    This  feature  is  implemented only 
for truss beam elements (*SECTION_BEAM, ELFORM = 3) with material *MAT_001 or 
for discrete beam elements (ELFORM = 6) with material *MAT_071. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BSID 
BSNID 
BSEID 
NELE 
LFED 
FPULL 
LMIN 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
F 
F 
F 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
BSID 
Beam Source ID.  A unique number has to be used. 
BSNID 
Source node ID. 
BSEID 
Source element ID. 
NELE 
LFED 
Number of elements to be pulled out. 
Beam element fed length (typical element initial length). 
FPULL 
Pull-out force.  
GT.0:  Constant value, 
LT.0:  Load  curve  ID = (-FPULL)  which  defines  pull-out  force 
as  a  function  of  time.    Either  *DEFINE_FUNCTION  or
*DEFINE_  CURVE_FUNCTION  (with  argument  TIME)
can be used. 
LMIN 
Minimum  beam  element  length,  see  notes  below.    One  to  two
tenth of the fed length LFED is usually a good choice. 
Remarks: 
The source node BSNID can be defined for itself or it can be part of another structure.  It 
is free to move in space during the simulation process.  Initially, the source node should 
have the same coordinates as one of the source element (BSEID) nodes, but not having 
the same ID.  If the pre-defined pull-out force FPULL is exceeded in the element next to
the source, beam material gets drawn out by increasing the length of the beam without 
increasing its axial force (equivalent to ideal plastic flow at a given yield force).  If more 
than the pre-defined length LFED is drawn  out, a new beam element is generated.  A 
new  beam  element  has  an  initial  undeformed  length  of  1.1 ×  LMIN.    The  maximum 
number  of  elements  NELE  times  the  fed  length  LFED  defines  the  maximum  cable 
length that can be pulled out from the source node.
The available option is: 
TITLE 
*ELEMENT_BEARING 
Purpose:    Define  a  bearing  between  two  nodes.    A  description  of  this  model  can  be 
found in Carney, Howard, Miller, and Benson [2014]. 
Title Card.  Additional card for title keyword Option. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
Remarks 
  Card 1 
Variable 
Type 
Default 
1 
ID 
I 
0 
2 
ITYPE 
I 
0 
3 
N1 
I 
0 
TITLE 
C 
none 
1 
4 
CID1 
I 
0 
8 
5 
N2 
I 
0 
6 
CID2 
I 
0 
7 
NB 
I 
0 
Material Properties Card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EBALL 
PRBALL 
ERACE 
PRRACE 
STRESL 
Type 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0
5 
6 
7 
8 
5 
6 
7 
8 
Geometry Card. 
  Card 3 
Variable 
Type 
1 
D 
F 
2 
DI 
F 
3 
DO 
4 
DM 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
Geometry Card 2. 
  Card 4 
Variable 
1 
A0 
Type 
F 
2 
BI 
F 
3 
BO 
F 
4 
PD 
F 
Default 
0.0 
0.0 
0.0 
0.0 
Preloading Card. 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IPFLAG 
XTRAN 
YTRAN 
ZTRAN 
XROT 
YROT 
Type 
I 
F 
F 
F 
F 
F 
Default 
00 
0.0 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
ID 
Bearing ID. 
ITYPE 
Bearing type: 
EQ.1: ball bearing 
EQ.2:  roller bearing 
N1 
Node on centerline of shaft (the shaft rotates).
VARIABLE   
DESCRIPTION
CID1 
N2 
CID2 
Coordinate  ID  on  shaft.    The  local  z  axis  defines  the  axis  of 
rotation. 
Node  on  centerline  of  bearing  (the  bearing  does  not  rotate).    It
should initially coincide with N1.  
Coordinate  ID  on  bearing.    The  local  z  axis  defines  the  axis  of 
rotation. 
NB 
Number of balls or rollers. 
EBALL 
Young’s modulus for balls or rollers. 
PRBALL 
Poisson’s ratio for balls or rollers. 
ERACE 
Young’s modulus for races. 
PRRACE 
Poisson’s ratio for races. 
STRESL 
Specified  value  of  the  bearing  stress  required  to  print  a  warning
message  that  the  value  has  been  reached.    If  it  is  0.0,  then  no
message is printed. 
D 
DI 
DO 
DM 
A0 
BI 
BO 
PD 
Diameter of balls or rollers. 
Bore inner diameter. 
Bore outer diameter. 
Pitch  diameter.    If  DM  is  not  specified,  it  is  calculated  as  the
average of DI and DO. 
Initial contact angle in degrees 
Inner  groove  radius  to  ball  diameter  ratio  for  ball  bearings  and
the roller length for roller bearings.. 
Outer race groove radius to ball diameter ratio.  Unused for roller
bearings. 
Total  radial  clearance  between  the  ball  bearings  and  races  when
no load is applied.
VARIABLE   
DESCRIPTION
IPFLAG 
Preload flag 
EQ.0:  no preload. 
EQ.1:  displacement preload specified. 
EQ.2:  force preload specified. 
XTRAN 
Displacement or force preload in the local x direction. 
YTRAN 
Displacement or force preload in the local y direction. 
ZTRAN 
Displacement or force preload in the local z direction. 
Angle (in radians) or moment preload in local x direction. 
Angle (in radians) or moment preload in local y direction. 
XROT 
YROT 
Remarks: 
1. 
If the bearing stress limit parameter, STRESL, is exceeded, a message is written 
to the messag and d3hsp files.  When this value is exceeded there is no change 
in element behavior.s 
2.  Use of double precision for solution stability is strongly suggested. 
3.  A realistic level of bearing damping (which can be included using *ELEMENT_-
DISCRETE and *MAT_DAMPER_VISCOUS) may be needed for solution stabil-
ity. 
4.  Bearing forces can be output in the brngout file, using *DATABASE_BEARING.
*ELEMENT_DIRECT_MATRIX_INPUT_{OPTION} 
Available options include: 
<BLANK> 
BINARY 
Purpose:  Define an element consisting of mass, damping, stiffness, and inertia matrices 
in  a  specified  file  which  follows  the  format  used  in  the  direct  matrix  input,  DMIG,  of 
NASTRAN.    The  supported  format  is  the  type  6  symmetric  matrix  in  real  double 
precision.   LS-DYNA  supports  both  the  standard  and  the  extended  precision  formats.  
The  binary  format  from  *CONTROL_IMPLICIT_MODES  or  *CONTROL_IMPLICIT_-
STATIC_CONDENSATION  is  another  input  option.    The  mass  and  stiffness  matrices 
are  required.   The  inertia  matrix  is  required  when  using  *LOAD_BODY_OPTION  to 
correctly  compute  the  action  of  a  prescribed  base  acceleration  on  the  superelement, 
otherwise  the  inertia  matrix  is  unused.   The  damping  matrix  is  optional.   The 
combination  of  these  matrices  is  referred  to  as  a  superelement.    Three  input  cards  are 
required for each superelement. 
The degrees-of-freedom for this superelement may consist of generalized coordinates as 
well was nodal point quantities.  Degrees-of-freedom, defined using *NODE input, are 
called  attachment  nodes.   Only  attachment  nodes  are  included  in  the  output  to  the 
ASCII and binary databases. 
The matrices for a given superelement can be of different order.   However, the explicit 
integration scheme requires the inversion of the union of the element mass matrix and 
nodal  masses  associated  with  attachment  nodes.    Any  degree  of  freedom  included  in 
the  other  (stiffness,  damping,  inertia)  matrices  but  without  nonzero  columns  in  the 
combined mass matrix will be viewed as massless and constrained not to move.  After 
deleting  zero  rows  and  columns  the  combined  mass  matrix  is  required  to  be  positive 
definite. 
The  inertia  matrix  is  required  to  have  3  columns  which  corresponds  to  the  3  global 
coordinates.  It is used to compute the forces acting on the superelement by multiplying 
the inertia matrix times the gravitational acceleration specified via *LOAD_BODY_OP-
TION. 
There  is  no  assumption  made  on  the  order  of  the  matrices  nor  the  sparse  matrix 
structure  of  the  element  matrices  except  that  they  are  symmetric  and  the  combined 
mass matrix is invertible as described above. 
Multiple  elements  may  be  input  using  *ELEMENT_DIRECT_MATRIX_INPUT.   They 
may share attachment nodes with other direct matrix input elements.  Only *BOUND-
ARY_PRESCRIBED_MOTION and global constraints imposed via*NODE or *BOUND-
ARY_SPC  on  attachment  nodes  can  be  applied  in  explicit  applications.   Implicit 
applications can have additional constraints on attachment nodes. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EID 
IFRMT 
Type 
I 
  Card 2 
1 
0 
2 
Variable 
Type 
3 
4 
5 
6 
7 
8 
FILENAME 
C 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MASS 
DAMP 
STIF 
INERT 
Type 
C 
C 
C 
C 
  VARIABLE   
DESCRIPTION
EID 
Super element ID. 
IFRMT 
Format: 
EQ.0: standard format 
NE.0:  extended precision format 
MASS 
DAMP 
Name  of  mass  matrix  in  the  file  defined  by  FILENAME.    This
filename  should  be  no  more  than  eight  characters  to  be
compatible with NASTRAN. 
Name of damping matrix in the file defined by FILENAME.  This
filename  should  be  no  more  than  eight  characters  to  be 
compatible with NASTRAN.
STIF 
*ELEMENT_DIRECT_MATRIX_INPUT 
DESCRIPTION
Name of stiffness matrix in the file defined by FILENAME.  This
filename  should  be  no  more  than  eight  characters  to  be
compatible with NASTRAN. 
INERT 
Name  of  inertia  matrix  in  the  file  defined  by  FILENAME.    This 
filename  should  be  no  more  than  eight  characters  to  be
compatible  with  NASTRAN.    This  file  must  be  present  when 
*LOAD_BODY is used to put gravitational forces on the model.
Available options include: 
<BLANK> 
LCO 
*ELEMENT 
Purpose:    Define  a  discrete  (spring  or  damper)  element  between  two  nodes  or  a  node 
and ground.  
An option, LCO, is available for using a load curve(s) to initialize the offset to avoid the 
excitation  of  numerical  noise  that  can  sometimes  result  with  an  instantaneous 
imposition  of  the  offset.    This  can  be  done  using  a  single  curve  at  the  start  of  the 
calculation or two curves where the second is used during dynamic relaxation prior to 
beginning the transient part.  In the latter case, the first curve would simply specify the 
offset as constant during time.  If the LCO option is active, a second card is read.   
Beam  type  6,  see  *ELEMENT_BEAM  and  SECTION_BEAM,  may  be  used  as  an 
alternative to *ELEMENT_DISCRETE and *SECTION_DISCRETE, and is recommended 
if the discrete element’s line of action is not node N1 to N2, i.e., if VID.NE.0.  
NOTE:  The discrete elements enter into the time step calcu-
lations.  Care must be taken to ensure that the nodal 
masses  connected  by  the  springs  and  dampers  are 
defined and unrealistically high stiffness and damp-
ing values must be avoided.  All rotations are in ra-
dians. 
Card 
1 
2 
3 
4 
5 
6 
7 
Variable 
EID 
PID 
N1 
N2 
VID 
Type 
I 
I 
I 
I 
I 
Default 
none  none  none
none 
0 
S 
F 
1. 
8 
PF 
I 
0 
9 
10 
OFFSET 
F
Offset Load Curve Card.  Additional card for LCO keyword option. 
  Card  2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
LCIDDR 
Type 
I 
I 
Default 
none 
none 
  VARIABLE   
DESCRIPTION
EID 
PID 
N1 
N2 
VID 
Element ID.  A unique number is required.  Since null beams are
created  for  visualization,  this  element  ID  should  not  be  identical
to  element  ID’s  defined  for  ELEMENT_BEAM  and  ELEMENT_-
SEATBELT. 
Part ID, see *PART. 
Nodal point 1. 
Nodal  point  2.    If  zero,  the  spring/damper  connects  node  N1  to 
ground. 
Orientation  option.    The  orientation  option  should  be  used
cautiously  since  forces,  which  are  generated  as  the  nodal  points
displace,  are  not  orthogonal  to  rigid  body  rotation  unless  the
nodes  are  coincident.. 
  The  type  6,  3D  beam  element,  is
recommended  when  orientation  is  required  with  the  absolute
value  of  the  parameter  SCOOR  set  to  2  or  3,  since  this  option
avoids rotational constraints. 
EQ.0: the  spring/damper  acts  along  the  axis  from  node  N1  to
N2, 
NE.0: the  spring/damper  acts  along  the  axis  defined  by  the
orientation vector, VID defined in the *DEFINE_SD_ORI-
ENTATION section. 
S 
PF 
Scale factor on forces. 
Print flag: 
EQ.0: forces are printed in DEFORC file, 
EQ.1: forces are not printed DEFORC file.
VARIABLE   
OFFSET 
DESCRIPTION
Initial  offset.    The  initial  offset  is  a  displacement  or  rotation  at
time zero.  For example, a positive offset on a translational spring
will  lead  to  a  tensile  force  being  developed at  time  zero.    Ignore 
this input if LCID is defined below. 
LCID 
Load  curve  ID  defining  the  initial OFFSET  as  a  function  of  time.
Positive  offsets  correspond  to  tensile  forces,  and,  likewise
negative offsets result in compressive forces. 
LCIDDR 
Load curve ID defining OFFSET as a function of time during the
dynamic relaxation phase.
*ELEMENT_DISCRETE_SPHERE_{OPTION} 
Available options include: 
<BLANK> 
VOLUME 
Purpose:    Define  a  discrete  spherical  element  for  discrete  element  method  (DEM) 
calculations.    Currently,  LS-DYNA’s  implementation  of  the  DEM  supports  only 
spherical  particles,  as  discrete  element  spheres  (DES).    Each  DES  consists  of  a  single 
node  with  its  mass,  mass  moment  of  inertia,  and  radius  defined  by  the  input  below.  
Initial  coordinates  and  velocities  are  specified  via  the  nodal  data.    The  element  ID 
corresponds to the ID of the node.  The discrete spherical elements are visualized in LS-
PrePost using the same options as the SPH elements. 
If  the  VOLUME  option  is  active,  the  fields  for  MASS  and  INERTIA  are  based  on  per 
unit density. 
Please  note,  the  DES  part  requires  *PART,  *SECTION,  and  *MAT  keywords.    The 
element type and formulation values in *SECTION are ignored.  DEM retrieves the bulk 
modulus from the *MAT input for coupling stiffness and time step size evaluation, and 
density from the *MAT input if VOLUME is used to calculate the proper mass.  *MAT_-
ELASTIC  and  *MAT_RIGID  are  most  commonly  used,  but  other  material  models  are 
also permissible. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID 
PID 
MASS/
VOLUME 
INERTIA 
RADIUS 
Type 
I 
I 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
NID 
PID 
DES Node ID. 
DES Part ID, see *PART.
VARIABLE   
MASS/ 
VOLUME 
DESCRIPTION
If  the  VOLUME  keyword  option  is  set,  then  VOLUME  and  the
mass is calculated from material density, 
Otherwise this entry is interpreted as mass. 
𝑀 = MASS × 𝜌mat. 
INERTIA 
Mass moment of inertia. 
If  the  VOLUME  option  is  active,  the  actual  inertia  is  calculated 
from material density, 
𝐼 = INERTIA × 𝜌mat.
RADIUS 
Particle  radius.    The  particle  radius  is  used  for  defining  contact
between particles.
*ELEMENT_GENERALIZED_SHELL 
Purpose:    Define  a  general  3D  shell  element  with  an  arbitrary  number  of  nodes.    The 
formulation  of  this  element  is  specified  in  *DEFINE_ELEMENT_GENERALIZED_-
SHELL,  which  is  specified  through  the  part  ID    and  the  section  ID  .  For an illustration of this referencing, see Figure 15-31.  Using this 
generalized  shell  implementation  allows  a  rapid  prototyping  of  new  shell  element 
formulations without further coding. 
The element formulation used in *SECTION_SHELL needs to be greater or equal than 
1000.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EID 
PID 
NMNP 
Type 
I 
I 
I 
Default 
none 
none 
none 
Connectivity  Cards.    Define  the  connectivity  of  the  element  by  specifying  NMNP-
nodes (up to eight nodes per card).  Include as many cards as needed.  For example, for 
NMNP = 10, the deck should include two additional cards. 
  Card 2 
Variable 
1 
N1 
Type 
I 
2 
N2 
I 
3 
N3 
I 
4 
N4 
I 
5 
N5 
I 
6 
N6 
I 
7 
N7 
I 
8 
N8 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
EID 
PID 
Element ID.  Chose a unique number with respect to other elements.
Part ID, see *PART. 
NMNP 
Number of nodes to define this element. 
Ni 
Nodal  point  i  (defined  via  *NODE)  to  define  connectivity  of  this
element.
Remarks: 
1.  For post-processing and the treatment of contact boundary conditions, the use 
of interpolation shell elements  is necessary.  
2.  The definition of the connectivity of the element is basically arbitrary but it has 
to be in correlation with the definition of the element formulation in *DEFINE_-
ELEMENT_GENERALIZED_SHELL. 
26
25
16
15
24
14
Connectivity of 
Generalized-Shell Element
Generalized-Shell Element
*ELEMENT_GENERALIZED_SHELL
$---+--EID----+--PID----+-NMNP----+----4----+----5----+----6----+----7----+----8
1 
11
$---+---N1----+---N2----+---N3----+---N4----+---N5----+---N6----+---N7----+---N8
16 
$---+---N9----+--Etc----+--Etc----+--Etc----+--Etc----+--Etc----+--Etc----+--Etc
15 
26 
24 
14 
25 
6 
*PART
Part for generalized shell
$---+--
PID----+SECID----+--MID----+----4----+----5----+----6----+----7----+----8
11
15
*SECTION_SHELL
$---+
SECID----ELFORM----+-SHRF----+--NIP----+----5----+----6----+----7----+----8
$---+---T1----+---T2----+---T3----+---T4----+----5----+----6----+----7----+----8
1001
15
1.0
*DEFINE_ELEMENT_GENERALIZED_SHELL
$---ELFORM---+---NGP----+-NMNP----+IMASS----+-FORM----+----6----+----7----+----8
0 
1001
4 
9 
...
Figure  17-3.    Example  of  the  connection  between  *ELEMENT_GENERAL-
IZED_SHELL and *DEFINE_ELEMENT_GENERALIZED_SHELL.
*ELEMENT_GENERALIZED_SOLID 
Purpose:    Define  a  general  3D  solid  element  with  an  arbitrary  number  of  nodes.    The 
formulation of this element is specified in *DEFINE_ELEMENT_GENERALIZED_SOL-
ID, which is referenced through the part ID  and the section ID .    For  an  illustration  of  this  referencing,  see  Figure  17-4.    Using  this 
generalized  solid  implementation  allows  a  rapid  prototyping  of  new  solid  element 
formulations without further coding. 
The  element  formulation  used  in  *SECTION_SOLID  needs  to  be  greater  or  equal  than 
1000.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EID 
PID 
NMNP 
Type 
I 
I 
I 
Default 
none 
none 
none 
Connectivity  Cards.    Define  the  connectivity  of  the  element  by  specifying  NMNP-
nodes (up to eight nodes per card).  Include as many cards as needed.  For example, for 
NMNP = 10, the deck should include two additional cards. 
  Card 2 
Variable 
1 
N1 
Type 
I 
2 
N2 
I 
3 
N3 
I 
4 
N4 
I 
5 
N5 
I 
6 
N6 
I 
7 
N7 
I 
8 
N8 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
EID 
PID 
Element ID.  Chose a unique number with respect to other elements.
Part ID, see *PART. 
NMNP 
Number of nodes to define this element. 
Ni 
Nodal  point  i  (defined  via  *NODE)  to  define  connectivity  of  this
element.
Remarks: 
1.  For post-processing the use of interpolation solid elements   is 
necessary.  
2.  The definition of the connectivity of the element is basically arbitrary but it has 
to be in correlation with the definition of the element formulation in *DEFINE_-
ELEMENT_GENERALIZED_SOLID. 
56
55
46
45
26
54
24
25
44
15
16
35
14
34
36
Connectivity of
Generalized-Solid Element
Generalized-Solid Element
*ELEMENT_GENERALIZED_SOLID
$---+--EID----+--PID----+-NMNP----+----4----+----5----+----6----+----7----+----8
11
18
56 
$---+---N1----+---N2----+---N3----+---N4----+---N5----+---N6----+---N7----+---N8
35
46 
$---+---N9----+--N10----+--N11----+--N12----+--N13----+--N14----+--N15----+--N16
24 
$---+--N17----+--N18----+--Etc----+--Etc----+--Etc----+--Etc----+--Etc----+--Etc
26 
55 
34 
25 
54 
36 
14 
44 
16 
45 
15 
5 
*PART
Part for generalized solid
$---+--PID----+SECID----+--MID----+----4----+----5----+----6----+----7----+----8
11
15
*SECTION_SOLID
$---+SECID----ELFORM----+--AET----+----4----+----5----+----6----+----7----+----8
1001
15
*DEFINE_ELEMENT_GENERALIZED_SOLID
$---ELFORM---+---NGP----+-NMNP----+IMASS----+----5----+----6----+----7----+----8
1001
18 
8 
Figure  17-4.    Example  of  the  connection  between  *ELEMENT_GENERAL-
IZED_SOLID and *DEFINE_ELEMENT_GENERALIZED_SOLID.
Available options include: 
<BLANK> 
OFFSET 
*ELEMENT_INERTIA 
Purpose:  to allow the lumped mass and inertia tensor to be offset from the nodal point.  
The nodal point can belong to either a deformable or rigid node. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
EID 
NID 
CSID 
Type 
I 
I 
I 
Default 
none  none  none 
Remarks 
1 
  Card 2 
1 
Variable 
IXX 
2 
IXY 
3 
IXZ 
4 
IYY 
5 
IYZ 
6 
7 
8 
IZZ 
MASS 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Remarks 
2 
2
Offset Card.  Additional card for offset keyword option.  
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
X-OFF 
Y-OFF 
Z-OFF 
Type 
F 
Default 
0. 
Remarks 
F 
0. 
2 
F 
0. 
2 
  VARIABLE   
DESCRIPTION
EID 
NID 
CSID 
IXX 
IXY 
IXZ 
IYY 
IYZ 
IZZ 
MASS 
X-OFF 
Y-OFF 
Z-OFF 
Element ID.  A unique number must be used. 
Node ID.  Node to which the mass is assigned. 
Coordinate system ID 
EQ.0: global inertia tensor 
GE.1: principal  moments  of  inertias  with  orientation  vectors
defined by Coordinate system CSID.  See *DEFINE_CO-
ORDINATE_SYSTEM  and  *DEFINE_COORDINATE_-
VECTOR. 
𝑥𝑥component of inertia tensor. 
𝑥𝑢 component of inertia tensor. 
𝑥𝑧 component of inertia tensor. 
𝑦𝑦 component of inertia tensor. 
𝑦𝑧 component of inertia tensor. 
𝑧𝑧 component of inertia tensor. 
Lumped mass 
𝑥-offset from nodal point. 
𝑦-offset from nodal point. 
𝑧-offset from nodal point.
*ELEMENT_INERTIA 
1.  The coordinate system cannot be defined for this element using the option, 
*DEFINE_COORDINATE_NODE. 
2. 
If  CSID  is  defined  then  IXY,  IXZ  and  IYZ  are  set  to  zero.    The  nodal  inertia 
tensor must be positive definite, i.e., its determinant must be greater than zero, 
since its inverse is required.  This check is done after the nodal inertia is added 
to the defined inertia tensor.
*ELEMENT_INTERPOLATION_SHELL 
Purpose:    With  the  definition  of  interpolation  shells,  the  stresses  and  other  solution 
variables  can  be  interpolated  from  the  generalized  shell  elements   
permitting the solution to be visualized using standard 4-noded shell elements with one 
integration  point  (one  value  of  each  solution  variable  per  interpolation  shell).    The 
definition  of  the  interpolation  shells  is  based  on  interpolation  nodes  . 
  The  connections  between  these  various 
keywords are illustrated in Figure 17-5. 
and 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EIDS 
EIDGS 
NGP 
Type 
I 
I 
I 
Default 
none 
none 
none 
Weighting Factor Cards.  These cards set the weighting factors used for interpolating 
the  solution  onto  the  center  of  this  interpolation  shell.    Set  one  weight  for  each  of  the 
NGP integration points.  Each card can accommodate 4 points; define as many cards as 
necessary.  As an example, for NGP = 10 three cards are required. 
  Card 2 
1 
Variable 
IP1 
2 
W1 
3 
IP2 
4 
W2 
5 
IP3 
6 
W3 
7 
IP4 
8 
W4 
Type 
I 
F 
I 
F 
I 
F 
I 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
EIDS 
DESCRIPTION 
Element ID of the interpolation shell.  This needs to coincide with a
proper  definition  of  a  4-noded  shell  element  (*ELEMENT_SHELL) 
using  interpolation  nodes  (*CONSTRAINED_NODE_INTERPOLA-
TION). 
EIDGS 
Element  ID  of  the  master  element  defined  in  *ELEMENT_GENER-
ALIZED_SHELL.
VARIABLE   
DESCRIPTION 
NGP 
Number of in-plane integration points of the master element. 
Integration  point  number  (1  to  NGP)  in  the  order  how  they  were 
defined in *DEFINE_ELEMENT_GENERALIZED_SHELL. 
Interpolation weight of integration point i. 
IPi 
Wi 
Remarks: 
1.  For  each  interpolation  shell  element,  one  single  value  (𝑣𝐼𝑆)  of  a  solution 
variable  is  interpolated  based  on  values  at  the  integration  points  (𝑣𝑖)  of  the 
master  element  (*ELEMENT_GENERALIZED_SHELL)  and  the  appropriate 
weighting  factors  (𝑤𝑖).    The  interpolation  is  computed  as  follows:  𝑣𝐼𝑆 =
𝑁𝐺𝑃
∑ 𝑤𝑖𝑣𝑖
𝑖=1
. 
2.  To  use  *ELEMENT_INTERPOLATION_SHELL,  ELFORM = 98  has  to  be  used 
in *SECTION_SHELL
26
25
15
II
IV
14
24
16
III
79
80
12
83
Connectivity of
Generalized-Shell Element
78
11
81
82
13
14
84
85
Generalized-Shell Element
(*ELEMENT_GENERALIZED_SHELL)
86
Integration Point
Interpolation Node
(*CONSTRAINED_NODE_INTERPOLATION)
Interpolation Element
(*ELEMENT_INTERPOLATION_SHELL)
*CONSTRAINED_NODE_INTERPOLATION
$---+--NID----+NUMMN----+----3----+----4----+----5----+----6----+----7----+----8
78
$---+--MN1----+---W1----+--MN2----+---W2----+--MN3----+---W3----+--MN4----+---W4
0.15
0.32 
0.18 
0.35 
26 
16 
25 
15 
*ELEMENT_SHELL
$--+-EID---+ PID---+- N1---+--N2---+--N3---+--N4---+--N5---+--N6---+--N7---+--N8
82 
33 
79 
78 
81
11
*PART
Part for interpolation shell
$---+--PID----+SECID----+--MID----+----4----+----5----+----6----+----7----+----8
33 
45 
*SECTION_SHELL
$---+SECID----ELFORM----+-SHRF----+--NIP----+----5----+----6----+----7----+----8
$---+---T1----+---T2----+---T3----+---T4----+----5----+----6----+----7----+----8
98
45
1.0
*ELEMENT_INTERPOLATION_SHELL
$-----EIDS---+-EIDGS----+--NGP----+----4----+----5----+----6----+----7----+----8
11
$---+--IP1---+----W1----+--IP2----+---W2----+--IP3----+---W3----+--IP4----+---W4
0.1
0.2 
0.5 
0.2 
1 
4 
2 
3 
Figure 17-5.  Example for *ELEMENT_INTERPOLATION_SHELL.
*ELEMENT_INTERPOLATION_SOLID 
Purpose:    With  the  definition  of  interpolation  solids,  the  stresses  and  other  solution 
variables  can  be  interpolated  from  the  generalized  solid  elements   
permitting the solution to be visualized using standard 8-noded solid elements with one 
integration  point  (one  value  of  each  solution  variable  per  interpolation  solid).    The 
definition  of  the  interpolation  solids  is  based  on  interpolation  nodes  . 
  The  connection  between  these  various 
keywords are illustrated in Figure17-6.  
and 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EIDS 
EIDGS 
NGP 
Type 
I 
I 
I 
Default 
none 
none 
none 
Weighting Factor Cards.  These cards set the weighting factors used for interpolating 
the  solution  onto  the  center  of  this  interpolation  solid.    Set  one  weight  for  each  of  the 
element’s  NGP  integration  points.    Each  card  can  accommodate  4  points;  define  as 
many cards as necessary.  As an example, for NGP = 10 three cards are required. 
  Cards 
1 
Variable 
IP1 
2 
W1 
3 
IP2 
4 
W2 
5 
IP3 
6 
W3 
7 
IP4 
8 
W4 
Type 
I 
F 
I 
F 
I 
F 
I 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
EIDS 
DESCRIPTION 
Element ID of the interpolation solid.  This needs to coincide with a
proper  definition  of  a  8-noded  solid  element  (*ELEMENT_SOLID) 
using  interpolation  nodes  (*CONSTRAINED_NODE_INTERPOLA-
TION).
VARIABLE   
EIDGS 
DESCRIPTION 
Element  ID  of  the  master  element  defined  in  *ELEMENT_GENER-
ALIZED_SOLID. 
NGP 
Number of integration points of the master element. 
Integration  point  number  (1  to  NGP)  in  the  order  how  they  were 
defined in *DEFINE_ELEMENT_GENERALIZED_SOLID. 
Interpolation weight of integration point i. 
IPi 
Wi 
Remarks: 
1.  For  each  interpolation  solid  element,  one  single  value  (𝑣𝐼𝑆)  of  a  solution 
variable  is  interpolated  based  on  values  at  the  integration  points  (𝑣𝑖)  of  the 
master  element  (*ELEMENT_GENERALIZED_SOLID)  and  the  appropriate 
weighting  factors  (𝑤𝑖).    The  interpolation  is  computed  as  follows:  𝑣𝐼𝑆 =
𝑁𝐺𝑃
∑ 𝑤𝑖𝑣𝑖
𝑖=1
2.  To use *ELEMENT_INTERPOLATION_SOLID, ELFORM = 98 has to be used in 
*SECTION_SOLID
10
VI
11
II
14
15
12
13
VII
VIII
IV
III
16
17
18
78
80
83
79
Connectivity of
Generalized-Solid Element
81
11
Generalized-Solid Element
(*ELEMENT_GENERALIZED_SOLID)
85
Integration Point
Interpolation Node
(*CONSTRAINED_NODE_INTERPOLATION)
Interpolation Element
(*ELEMENT_INTERPOLATION_SOLID)
82
86
84
87
88
12
89
*ELEMENT_SOLID
$--+-EID---+ PID---+- N1---+--N2---+--N3---+--N4---+--N5---+--N6---+--N7---+--N8
11
33
$--+--N1---+--N2---+- N3---+--N4---+--N5---+--N6---+--N7---+--N8---+--N9---+-N10
78 
79 
86 
81 
83 
85 
80 
82
*PART
Part for interpolation solid
$---+--PID----+SECID----+--MID----+----4----+----5----+----6----+----7----+----8
33 
45 
*SECTION_SOLID
$---+SECID----ELFORM----+--AET----+----4----+----5----+----6----+----7----+----8
45
98
*ELEMENT_INTERPOLATION_SOLID
$-----EIDS---+-EIDGS----+--NGP----+----4----+----5----+----6----+----7----+----8
11
$---+--IP1---+----W1----+--IP2----+---W2----+--IP3----+---W3----+--IP4----+---W4
0.07
$---+--IP5---+----W5----+--IP6----+---W6----+--IP7----+---W7----+--IP8----+---W8
0.03
0.08 
0.12 
0.07 
0.13 
0.30 
0.20 
4 
8 
5 
1 
3 
7 
2 
6 
Figure 17-6.  Example for *ELEMENT INTERPOLATION SOLID.
*ELEMENT 
Purpose:    This  feature  models  a  lancing  process  during  a  metal  forming  process  by 
trimming along a curve.  Two types of lancing, instant and progressive, are supported.  
This  keyword  is  used  together  with  *DEFINE_CURVE_TRIM_3D,  and  only  applies  to 
shell  elements.    The  lanced  scraps  can  be  removed  (trimming)  during  or  after  lancing 
when used in conjunction with *DEFINE_LANCE_SEED_POINT_COORDINATES, see 
Trimming. 
The  element  lancing  feature  is  supported  in  LS-PrePost  4.3,  under  Application  → 
MetalForming → Easy Setup. 
For  each  trim  include  an  additional  card.    This  input  ends  at  the  next  keyword  (“*”) 
card. 
  Card 1 
1 
2 
3 
4 
Variable 
IDPT 
IDCV 
IREFINE 
SMIN 
Type 
I 
I 
Default 
none 
none 
I 
1 
F 
5 
AT 
F 
6 
7 
8 
ENDT 
NTIMES 
CIVD 
F 
I 
I 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
IDPT 
A flag to indicate if a part to be lanced is a part or a part set. 
GT.0: IDPT is the PID of a part to be lanced, see *PART. 
LT.0:  the  absolute  value 
in
*SET_PART_LIST.    This  option  allows  the  lancing  to  be 
performed across a tailor-welded line. 
the  part  set 
ID,  as 
is 
IDCV 
IREFINE 
A load curve ID (the variable TCID in *DEFINE_CURVE_TRIM_-
3D)  defining  a  lancing  route  .    XYZ  format 
(TCTYPE = 1) has always been supported, however, IGES format
(TCTYPE = 2) is not supported until Revision 110246. 
Set  IREFINE = 1  to  refine  elements  along  lancing  route  until  no
adapted nodes exist in the neighborhood.  This feature result in a
more  robust  lancing  in  the  form  of  improved  lancing  boundary.
Available starting in Revision 107708.  Values greater than “1” are
not  allowed.    See  Figure  17-15  for  an  example  of  the  mesh 
refinement.
Minimum  element  characteristic  length  to  be  refined  to,  to  be
supported  in  the  future.    Currently,  one  level  of  refinement  will 
be automatically made. 
Activation  time  for  lancing  operation.    This  variable  needs  to  be
defined  for  both  instant  and  progressive  lancing  types  .    If  CIVD  is  defined,  AT  becomes  the  distance  from
punch home position. 
Lancing  end  time  (for  progressive  lancing  only).    If  CIVD  is 
defined, ENDT becomes the distance from punch home position.
Do not define for instant lancing. 
A  progressive  lancing  operation  is  evenly  divided  into  NTIMES
segments between AT and ENDT; within each segment lancing is
done instantly.   Do not define for instant lancing. 
ID 
load 
curve 
(LCID) 
keyword
The 
under 
the
*BOUNDARY_PRESCRIBED_MOTION_RIGID 
  velocity)  of  the  tool,  with  VAD = 0. 
kinematics  (time  vs. 
Furthermore,  when  this  variable  is  used,  AT  and  ENDT  will 
become  the  distances  from  punch  bottom  position.    See  an
example  inLance-trimming  with  negative  IDPT,  IGES  curve,  a
seed node and CIVD. 
the 
to  define 
*ELEMENT 
  VARIABLE   
SMIN 
AT 
ENDT 
NTIMES 
CIVD 
Remarks: 
Lancing  the  blank  during  forming  at  strategic  locations  under  controlled  conditions 
alleviates thinning and necking of sheet metal panels.  Typically, the blank is lanced in 
the last few millimeters before the punch reaches its home position.  Being an unstable 
process,  lancing  is  not  favored  by  all  stampers,  nevertheless  many  users  have  devised 
process which would be impossible without lancing. 
The  benefits  of  lancing  are  illustrated  in  Figure  17-7.    In  this  figure  two  closed-loop 
holes  are  instantly  lanced  each  along  the  C-pillar  top  (window  opening  area)  and 
bottom (window regulator area) to improve the formability at those two corners.  The 
right panel of Figure 17-7 is lanced and suffers less thinning compared to the no-lancing 
case,  which  is  shown  in  the  left-panel.    This  keyword  offers  two  types  of  lancing 
operations: 
1. 
Instant  lancing.    Instant  lancing  cuts  the  sheet  metal  once  along  the  defined 
curve at a time specified in the AT field.
2.  Progressive  lancing.    The  cut  is  spatially  divided  into  NTIMES  sub-lances 
traveling along the curve in the direction of definition.  See Figure 17-10.  Pro-
gressive  lancing  starts  at  AT  and  ends  at  ENDT  thereby  achieving  a  gradual 
and even release along the curve. 
Modeling information: 
Some modeling guidelines and limitations are listed below: 
1.  Both  closed-loop  (Figure  17-8)  and  open-loop  (Figure  17-9)  lancing  curves  are 
supported.  Lancing curve may not cross each other, and cross itself. 
2.  Since  progressive  lancing  starts  from  the  beginning  of  the  curve  and  proceeds 
towards  the  end,  the  direction  of  the  curve  needs  to  be  defined  to  match  the 
direction of the physical cut (Figure 17-10).  The direction can be set using LS-
PrePost.  The menu option GeoTol→ Measure with the Edge box checked can be 
used to show the direction of the curve.  If the direction is not as desired, GeoTol 
→ Rever can be used to reverse the direction. 
3.  The effect of NTIMES can be seen in Figure 17-11.  Compared with NTIMES of 
6, setting NTIMES to a value of 20 results in a smoother lancing boundary and 
less stress concentration along the separated route. 
4.  Although  the  IGES  format  curve  is  supported  in  the  keyword  *DEFINE_-
CURVE_TRIM_3D, curves defined with the keyword and used for lancing must 
be specified using only the XYZ format (TCTYPE = 1 or 0).  The manual entry in 
the  keyword  manual  for  the  *INTERFACE_BLANKSIZE_DEVELOPMENT 
keyword outlines a procedure for converting an IGES file into the required XYZ 
format.    Note  the  IGES  format  support  for  lancing  is  enabled  starting  in  Revi-
sion 110246. 
5.  The  first  two  points  and  as  well  as  the  last  two  points  of  the  any  progressive 
lancing curve must be separated so that LS-DYNA can correctly determine the 
direction of the curve. 
6.  The lancing curve needs to be much longer than the element sizes in the lancing 
area. 
7.  To  prevent  mesh  distortion  at  the  end  of  the  lancing  route  ENDT  must  be 
defined  to  be  less  than  the  simulation  completion  time  (slightly  less  is  suffi-
cient). 
8.  As  currently  implemented,  lancing  is  assumed  to  be  in  the  Z-direction.    This 
keyword  does  not  model  lancing  along  the  draw  wall  with  surface  normals 
nearly perpendicular to the Z-axis.
9.  Tailor-welded  blanks  are  supported;  however,  the  lancing  route  should  not 
cross the laser line, as currently only one part can be defined with one lancing 
curve. 
10.  Both  *PARAMETER  and  *PARAMETER_EXPRESSION  are  supported  for  BT 
and DT as of Revision 92335.  This makes it possible for users to input distance 
from  punch  home  as  onset  of  the  lancing.    Refer  to  Figure  17-13,  where  a 
punch’s velocity profile is shown, the lancing activation time “at”, is calculated 
based on the distance to home, “dhome” (the shaded area), punch travel veloci-
ty  “vdraw”,  and  total  simulation  time  “ENDTIME”.    The  variable  CIVD  imple-
mented in Rev 110173 removes the need for the calculation of AT  from punch 
distance to home.  
11.  Mesh  adaptivity  (*CONTROL_ADAPTPIVE  and  the  parameter  “ADPOPT” 
under *PART) must be turned on during lancing. 
12.  All  trim  curves  used  to  define  lancing  routes  (*DEFINE_CURVE_TRIM_3D) 
must be placed after all other curves in the input deck.  Furthermore, no curves 
defined by *DEFINE_CURVE_TRIM_3D that are not used for lancing should be 
present anywhere in the input deck.  Note this restriction is removed starting in 
Revision 110316. 
13.  Only *DEFINE_CURVE_TRIM_3D (not _NEW) is supported.  If defined curve 
is far away from the blank it will be projected in Z-direction onto the blank. 
Application example: 
A partial deck implementing instant lancing is listed below.  A blank having a PID of 8 
is  being  lanced  along  curves  #119  and  #202  instantly  at  0.05  and  0.051  seconds, 
respectively. 
*ELEMENT_LANCING 
$     IDPT      IDCV   IREFINE      SMIN        AT      ENDT    NTIMES 
         8       119                        0.0500     
         8       202                        0.0510     
*DEFINE_CURVE_TRIM_3D 
$#    tcid    tctype      tflg      tdir     tctol      toln     nseed 
       119         1         1               0.100         1  
$#                cx                  cy                  cz 
           172.99310           42.632320           43.736160 
           175.69769          -163.08299           46.547531 
           177.46982          -278.03793           49.138161 
           186.82404          -303.67191           51.217964 
           205.16177          -315.33484           53.299248 
               ⋮                   ⋮                    ⋮ 
*DEFINE_CURVE_TRIM_3D 
$#    tcid    tctype      tflg      tdir     tctol      toln     nseed 
       202         1         1               0.100         1  
$#                cx                  cy                  cz 
           187.46982          -578.73793           89.238161 
           168.88404          -403.97191           61.417964
215.18177          -215.03484           73.899248 
               ⋮                   ⋮                    ⋮ 
A  partial  keyword  deck  implementing  two  progressive  lances  is  listed  below.    Both 
lances travel along paths starting at the same coordinate value.  A sheet blank having a 
part  ID  of  9  is  progressively  lanced  along both  curves  (IDCV = 1  and  2)  as  defined  by 
*DEFINE_CURVE_TRIM_3D.    Both  lancing  operations  commence  at  0.05  seconds  and 
finish at 0.053 seconds with 20 cuts along each curve in opposite direction.  The lancing 
results  are  shown  in  Figure  17-12.    Note  that  the  termination  time  is  53.875  seconds, 
which is slightly larger than the ENDT. 
*ELEMENT_LANCING 
$     IDPT      IDCV   IREFINE      SMIN        AT      ENDT    NTIMES 
         9         1                        0.0500   5.3E-02        20 
         9         2                        0.0500   5.3E-02        20 
*DEFINE_CURVE_TRIM_3D 
$#    tcid    tctype      tflg      tdir     tctol      toln     nseed 
         1         1         1               0.100         1  
$#                cx                  cy                  cz 
           172.99310           42.632320           43.736160 
           175.69769          -163.08299           46.547531 
           177.46982          -278.03793           49.138161 
           186.82404          -303.67191           51.217964 
           205.16177          -315.33484           53.299248 
           223.13152          -308.03534           54.193089 
           234.96263          -290.49695           54.885273 
           222.03900          -270.08289           53.163551 
           199.31226          -251.27985           50.401234 
               ⋮                   ⋮                    ⋮ 
*DEFINE_CURVE_TRIM_3D 
         2         1         1               0.100         1  
$#                cx                  cy                  cz 
           172.99310           42.632320           43.736160 
           171.33121            47.22141           42.513367 
           171.28690           128.84601           43.032799 
           176.89932           149.39539           43.495331 
           192.41418           159.53757           44.756699 
           208.39861           158.93469           45.878036 
           218.10101           149.34409           47.128345 
           218.34503           135.23810           47.682144 
           209.05414           122.82422           46.616959 
           190.19659           117.66074           44.858204 
               ⋮                   ⋮                    ⋮ 
Trimming after lancing: 
removed 
lancing  simulation. 
(trimming)  after  a 
As shown in Figure 17-14 and the following partial keyword file, the lanced scraps can 
  An  extra  keyword, 
be 
*DEFINE_LANCE_SEED_POINT_COORDINATES is needed to define the portion that 
would  remain  after  the  lancing  and  trimming.    It  should  be  obvious  that  the  lancing 
curve defined by *DEFINE_CURVE_TRIM_3D must form a closed loop.  The following 
example  will  trim  a  part  ID  9  with  a  fully  enclosed  lancing  curve  #1,  at  time = 0.049 
seconds.    Since  the  termination  time  is  0.0525  seconds,  the  scrap  will  be  deleted 
(trimmed off) before the simulation ends.  The scrap, enclosed by the curve, is located
outside 
*DEFINE_LANCE_SEED_POINT_COORDINATES (starting in Revision 107262). 
defined 
node, 
seed 
the 
of 
by 
*CONTROL_TERMINATION 
0.0525 
*ELEMENT_LANCING 
$     IDPT      IDCV   IREFINE      SMIN        AT      ENDT    NTIMES 
         9         1                        0.0490 
*DEFINE_CURVE_TRIM_3D 
$#    tcid    tctype      tflg      tdir     tctol      toln     nseed 
         1         1         1               0.100         1  
$#                cx                  cy                  cz 
           172.99310           42.632320           43.736160 
           175.69769          -163.08299           46.547531 
           177.46982          -278.03793           49.138161 
           186.82404          -303.67191           51.217964 
           205.16177          -315.33484           53.299248 
           223.13152          -308.03534           54.193089 
               ⋮                   ⋮                    ⋮ 
           172.99310           42.632320           43.736160 
           172.99310           42.632320           43.736160 
*DEFINE_LANCE_SEED_POINT_COORDINATES 
$    NSEED        X1       Y1         Z1       X2        Y2        Z2 
         1    -289.4    98.13   2354.679 
This  feature  also  makes  it  possible  to  combine  the  trimming  process  together  with  a 
forming simulation, saving a trimming step in a line-die process simulation by skipping 
writing  out  a  formed  dynain  file  and  reading  in  the  same  file  for  the  trimming 
simulation. 
Lance-trimming with negative IDPT, IGES curve, a seed node and CIVD: 
The following partial keyword input shows instant lance-trimming across the weld line 
of a tailor-welded blank using the part set ID “blksid” 100, which consists of PIDs 1 and 
9.  The part set ID used for *ELEMENT_LANCING input is “idpt”, which is set as the 
negative  of  blksid  (-100).    The  lance-trimming  curve  ID  1117  is  defined  using  the  file 
lance4.iges in IGES format (TCTYPE = 2).  The variable CIVD is referred to load curve 
ID 12, which is the kinematic curve for the punch.  The lancing starts at 15.5 mm away 
from punch bottom (AT = 15.5).  A lance seed coordinate (-382.0, -17.0, 76.0) is defined 
using the keyword *DEFINE_LANCE_SEED_POINT_COORDINATES, resulting in the 
lanced scrap piece being removed after lancing. 
*PARAMETER 
I blk1pid          1 
I blk2pid          9 
I blksid         100 
*SET_PART_LIST 
&blksid 
&blk1pid    &blk2pid 
*PARAMETER_EXPRESSION 
I idpt        -1*blksid 
*ELEMENT_LANCING 
$     IDPT      IDCV   IREFINE      SMIN        AT      ENDT    NTIMES      CIVD 
     &idpt      1117         1                15.5                          1115 
*DEFINE_CURVE_TRIM_3D
$#    tcid    tctype      tflg      tdir     tctol      toln    nseed1    nseed2 
      1117         2         1         0    0.1000         0 
lance4.iges 
*DEFINE_LANCE_SEED_POINT_COORDINATES 
$     NSUM        X1        Y1        Z1        X2        Y2        Z2 
         1  -382.000   -17.000      76.0 
*BOUNDARY_PRESCRIBED_MOTION_RIGID 
$   TYPEID       DOF       VAD      LCID        SF       VID     DEATH     BIRTH 
  &udiepid         3         0      1113                      &clstime 
  &bindpid         3         0      1114                      &clstime 
  &udiepid         3         0      1115                      &endtime  &clstime 
  &bindpid         3         0      1115                      &endtime  &clstime 
Revision information: 
This  feature  is  available  starting  in  Revision  83562  for  SMP  and  in  Revision  94383  for 
MPP,  in  explicit  dynamic  calculation  only.    Later  revisions  incorporate  various 
improvements.  The list below provides revision information: 
14.  Revision 92335: support of *PARAMETER and *PARAMETER_EXPRESSION. 
15.  Revision 94383: MPP support of lancing is available. 
16.  Revision 107708: support IREFINE = 1. 
17.  Revision 107262: lancing with trimming is supported. 
18.  Revision 110173: CIVD is supported, and AT and ENDT become distances from 
punch home if CIVD is activated. 
19.  Revision 110177: support negative IDPT for part set ID, enabling lancing across 
the laser welded line. 
20.  Revision 110246: lancing curve definition in IGES format is supported.
Area thinning reduced by 
neighboring lanced hole
Thinning (%)
20.0
18.0
16.0
14.0
12.0
10.0
8.0
6.0
4.0
2.0
 0.0
Area thinning reduced by 
neoghboring lanced hole
Areas of high thinning (in blue) 
- without lancing
Thinning contour with lancing in 
upper and lower C-pillar corners 
Figure 17-7.  Thinning improvement on a door inner as a result of lancing at
the upper and lower corner of the C-pillar. 
Figure 17-8.  Instant lancing – closed-loop hole.  The left mesh is immediately
after AT while the right one is at punch home.
Figure 17-9.  Instant lancing – open-loop hole.  The left mesh is immediately
after AT while the right one is at punch home. 
ENDT
Curve direction
. . .
AT
Figure  17-10.    Progressive  lancing  -  defining  AT,  ENDT,  NTIMES,  curve
direction; mesh separation progression during progressive lancing.
NTIMES=6
NTIMES=20
Figure 17-11.  More NTIMES gives smoother lancing boundary and less stress
concentration. 
curve #2 direction
curve #1 direction
same starting point
Figure  17-12.    Progressive  lancing  –  multiple  lancing  starting  from  the  same
coordinates.
Tool velocity
vdraw
AT
dhome
Time
ENDTIME
*PARAMETER_EXPRESSION
R dhome       12.5
R at                ENDTIME-dhome/vdraw
*ELEMENT_LANCING
$ IDPT           IDCV         IREFINE          SMIN          AT
          9               112                                                       &at    
Figure 17-13.  An example of defining lancing activation time AT using tool’s
distance to home. 
Time = 0.049
Scrap deleted
Time = 0.0525
Scrap kept
Thinning (%)
20.0
18.0
16.0
14.0
12.0
10.0
8.0
6.0
4.0
2.0
-0.0
Seed point defines part that 
remains post trimming
Lancing with trimming 
at t=0.049 sec
Lancing only
Figure 17-14.  Lancing with trimming
Lanced mesh prior to 
Revision 107708
Improved lanced boundary mesh with 
IREFINE=1 after Revision 107708
Figure  17-15.    Set  IREFINE = 1  (>Revision  107708)  for  improved  lanced
boundary.
Available options include: 
<BLANK> 
NODE_SET 
*ELEMENT 
Purpose:    Define  a  lumped  mass  element  assigned  to  a  nodal  point  or  equally 
distributed to the nodes of a node set. 
(Note:  NODE_SET option is available starting with the R3 release of Version 971.) 
Card 
1 
Variable 
EID 
Type 
I 
2 
ID 
I 
Default 
none  none 
3 
4 
5 
6 
7 
8 
9 
10 
MASS 
PID 
F 
0. 
I 
none 
  VARIABLE   
DESCRIPTION
EID 
ID 
MASS 
Element ID.  A unique number is recommended.  The nodes in a
node set share the same element ID. 
Node ID or node set ID if the NODE_SET option is active.  This is 
the node or node set to which the mass is assigned.   
Mass  value.    When  the  NODE_SET  option  is  active,  the  mass  is 
equally distributed to all nodes in a node set. 
PID 
Part ID.  This input is optional. 
Remarks: 
1. 
Kinetic energy of lumped mass elements is output as kinetic energy of part 0 in 
matsum  (*DATABASE_MATSUM)  if  IERODE  is  set  to  1  on  *CONTROL_OUT-
PUT.
*ELEMENT_MASS_MATRIX_{OPTION} 
Available options include: 
<BLANK> 
NODE_SET 
Purpose:  Define a 6 × 6 symmetric nodal mass matrix assigned to a nodal point or each 
node within a node  set.  A node may not be included in more than one *ELEMENT_-
MASS_MATRIX(_NODE_SET) command. 
  Card 1 
1 
Variable 
EID 
Type 
I 
2 
ID 
I 
Default 
none 
none 
  Card 2 
1 
2 
3 
CID 
I 
0 
3 
4 
5 
6 
7 
8 
4 
5 
6 
7 
8 
Variable 
M11 
M21 
M22 
M31 
M32 
M33 
M41 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
M42 
M43 
M44 
M51 
M52 
M53 
M54 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
M55 
M61 
M62 
M63 
M64 
M65 
M66 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
EID 
ID 
CID 
Mij 
Element ID.  A unique number is recommended.  The nodes in a
node set share the same element ID. 
Node ID or node set ID if the NODE_SET option is active.  This is 
the node or node set to which the mass is assigned.   
Local  coordinate  ID  which  defines  the  orientation  of  the  mass 
matrix 
The ijth term of the symmetric mass matrix.  The lower triangular
part of the matrix is defined.
Available options include: 
<BLANK> 
SET  
*ELEMENT_MASS_PART 
  Define  additional  non-structural  mass  to  be  distributed  by  an  ar-
Purpose: 
ea (shell) / volume (solid) or mass weighted distribution to all nodes of a given part, or 
part  set,  ID.    As  an  option,  the  total  mass  can  be  defined  and  the  additional  non-
structural  mass  is  computed.    This  option  applies  to  all  part  ID's  defined  by  shell  and 
solid elements. 
Card 
Variable 
1 
ID 
Type 
I 
Default 
none 
2 
3 
4 
5 
6 
7 
8 
9 
10 
ADDMASS 
FINMASS 
LCID 
MWD 
F 
0. 
F 
0. 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
ID 
Part or part set ID if the SET option is active.  A unique number
must be used. 
ADDMASS 
FINMASS 
Added  translational  mass  to  be  distributed  to  the  nodes  of  the
part ID or part set ID.  Set to zero if FINMASS is nonzero.  Since
the additional mass is not included in the time step calculation of
the elements in the PID or SID, ADDMASS must be greater than 
zero if FINMASS is zero. 
Final  translational  mass  of  the  part  ID  or  part  set  ID.    The  total
mass of the PID or SID is computed and subtracted from the final
mass of the part or part set to obtain the added translational mass,
which  must  exceed  zero.    Set  FINMASS  to  zero  if  ADDMASS  is 
nonzero.  FINMASS is available in the R3 release of version 971. 
LCID 
Optional load curve ID to scale the added mass at time = 0.  This 
curve defines the scale factor as a function versus time.  The curve
must  start  at  unity  at  t = 0.    This  option  applies  to  deformable 
bodies only.
VARIABLE   
MWD 
DESCRIPTION
Optional  flag  for  mass-weighted  distribution,  valid  for  SET 
option only: 
EQ.0: non-structural  mass 
is 
distributed 
by 
ar-
ea(shell)/volume(solid) weighted distribution, 
EQ.1: non-structural  mass  is  distributed  by  mass  weighted,
area*density*thickness(shell)/volume*density(solid), 
distribution. 
Mixed uses with MWD for the same part should be avoided.
Purpose:  Define a null beam element for visualization. 
*ELEMENT_PLOTEL 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
EID 
N1 
N2 
Type 
I 
I 
I 
Default 
none  none  none 
Remarks 
1 
  VARIABLE   
DESCRIPTION
Element ID.  A unique number must be used. 
Nodal point (end) 1. 
Nodal point (end) 2. 
EID 
N1 
N2 
Remarks: 
1.  Part ID, 10000000, is assigned to PLOTEL elements. 
2.  PLOTEL element ID’s must be unique with respect to other beam elements.
Purpose:  Define a seat belt element. 
*ELEMENT 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
EID 
PID 
N1 
N2 
SBRID 
SLEN 
N3 
N4 
Type 
I 
I 
I 
I 
I 
F 
Default 
none  none  none  none  none 
0.0 
Remarks 
1 
2 
I 
0 
I 
0 
3 
  VARIABLE   
DESCRIPTION
EID 
PID 
N1 
N2 
SBRID 
SLEN 
N3 
Element ID.  A unique number is required.  Since null beams are
created  for  visualization,  this  element  ID  should  not  be  identical
to  element  ID’s  defined  for  ELEMENT_BEAM  and  ELEMENT_-
DISCRETE. 
Part ID 
Node 1 ID 
Node 2 ID 
Retractor ID, see *ELEMENT_SEATBELT_RETRACTOR. 
Initial slack length 
Optional  node  3  ID.    When  N3 > 0  and  N4 > 0,  the  elements 
becomes  a  shell  seat  belt  element.    The  thickness  of  the  shell
seatbelt  is  defined  in  *SECTION_SHELL,  not  in  *SECTION_-
SEATBELT.    The  shell-type  seatbelt  must  be  of  a  rectangular 
shape  as  shown  in  Figure  17-16  and  contained  in  a  logically 
regular mesh. 
N4 
Node 4 ID, which is required if and only if N3 is defined.
slipring
retractor
Top view:
SN5
SRE14
SRE24
SRE13
SN4
SN3
SRE23
SRE12
SRE22
SN2
SRE11
SRE21
SN1
RN5
RE4
RN4
RE3
RN3
RE2
RN2
RE1
RN1
Figure 17-16.  Definition of seatbelt shell elements.  The ordering of the nodes
and  elements  are  important  for  seatbelt  shells.    See  the  input  descriptions  for
SECTION_SHELL,  ELEMENT_SEATBELT_RETRACTOR  and  ELEMENT_SEAT-
BELT_SLIPRING. 
Remarks: 
1.  The  retractor  ID  should  be  defined  only  if  the  element  is  initially  inside  a 
retractor, see *ELEMENT_SEATBELT_RETRACTOR. 
2.  Belt  elements  are  single  degree  of  freedom  elements  connecting  two  nodes.  
When the strain in an element is positive (i.e.  the current length is greater then 
the  unstretched  length),  a  tension  force  is  calculated  from  the  material  charac-
teristics and is applied along the current axis of the element to oppose further 
stretching.    The  unstretched  length  of  the  belt  is  taken  as  the  initial  distance 
between the two nodes defining the position of the element plus the initial slack 
length.
3.  Seatbelt shell elements are a new feature in version 971 and must be used with 
caution.  The seatbelt shells distribute the loading on the surface of the dummy 
more  realistically  than  the  two  node  belt  elements.    For  the  seatbelt  shells  to 
work with sliprings and retractors it is necessary to use a logically regular mesh 
of quadrilateral elements.  A seatbelt defined by a part ID must not be disjoint. 
4. 
1D and 2D seatbelt elements may not share the same material ID.
*ELEMENT_SEATBELT_ACCELEROMETER 
Purpose:  This keyword command defines an accelerometer.  Contrary to the keyword 
name,  an  accelerometer  need  not  be  associated  with  a  seat  belt.    The  accelerometer  is 
fixed to a rigid body containing the three nodes defined below.  An accelerometer will 
exhibit  considerably  less  numerical  noise  than  a  deformable  node,  thereby  reporting 
more meaningful data to the user.  Whenever computed accelerations are compared to 
experimental  data,  or  whenever  computed  accelerations  are  compared  between 
different runs, this feature is essential. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SBACID 
NID1 
NID2 
NID3 
IGRAV 
INTOPT 
MASS 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
F 
0. 
  VARIABLE   
DESCRIPTION
SBACID 
Accelerometer ID.  A unique number must be used. 
NID1 
NID2 
NID3 
Node 1 ID 
Node 2 ID 
Node 3 ID 
IGRAV 
Gravitational accelerations due to body force loads. 
EQ.-6:  𝑧 and 𝑥 components removed from acceleration output 
EQ.-5:  𝑦  and  𝑧  components  removed  from  acceleration  output
EQ.-4:  𝑥 and 𝑦 components removed from acceleration output 
EQ.-3:  𝑧 component removed from acceleration output 
EQ.-2:  𝑦 component removed from acceleration output 
EQ.-1:  𝑥 component removed from acceleration output 
EQ.0:  all components included in acceleration output 
EQ.1:  all components removed from acceleration output 
GT.1:  IGRAV  is  a  curve  ID  defining  the  gravitation-flag 
versus  time.    The  ordinate  values,  representing  the
VARIABLE   
DESCRIPTION
gravitation-flag, can be -6, -5, -4, -3, -2, -1, 0 or 1, as de-
scribed above.  For example, a curve with 4 data points
of  (0.,1),  (10.,1),  (10.000001,0),  (200.,0)  sets  gravitation
flag  to  be  1  when  time  ≤  10,  and  0  when  time > 10.    In 
other  words,  all  components  of  gravitational  accelera-
tions  are  removed  when  time  ≤  10.,  and  then  included 
when time > 10.0. 
Integration  option.    If  the  accelerometer  undergoes  rigid  body
translation without rotation this option has no effect; however, if
rotation occurs, INTOPT affects how translational velocities (and 
displacements)  are  calculated.    Note  that  the  acceleration  values
written to the nodout file are unaffected by INTOPT. 
EQ.0:  velocities  are  integrated  from  the  global  accelerations
and transformed into the local system of the accelerome-
ter.   
EQ.1:  velocities  are 
integrated  directly 
from 
the 
local
accelerations of the accelerometer. 
Optional  added  mass  for  accelerometer.      This  mass  is  equally
distributed  to  nodal  points  NID1,  NID2,  and  NID3.    This  option
avoids  the  need  to  use  the  *ELEMENT_MASS  keyword  input  if 
additional mass is required. 
INTOPT 
MASS 
Remarks: 
The presence of the accelerometer means that the accelerations and velocities of node 1 
will be output to all output files in local instead of global coordinates. 
The local coordinate system is defined by the three nodes as follows: 
1. 
2. 
local 𝐱 from node 1 to node 2, 
local  𝐳  perpendicular  to  the  plane  containing  nodes,  1,  2,  and  3  (𝐳 = 𝐱 × 𝐚), 
where a is from node 1 to node 3), 
3. 
local 𝐲 = 𝐳 × 𝐱. 
The three nodes should all be part of the same rigid body.  The local axis then rotates 
with the body.
*ELEMENT_SEATBELT_PRETENSIONER 
Purpose:    Define  seat  belt  pretensioner.    A  combination  with  sensors  and  retractors  is 
also possible. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SBPRID 
SBPRTY 
SBSID1 
SBSID2 
SBSID3 
SBSID4 
Type 
Default 
I 
0 
I 
0 
Remarks 
  Card 2 
1 
2 
I 
0 
1 
3 
I 
0 
I 
0 
I 
0 
4 
5 
6 
7 
8 
Variable 
SBRID 
TIME 
PTLCID 
LMTFRC 
Type 
Default 
I 
0 
F 
0.0 
I 
0 
F 
0 
Remarks 
  VARIABLE   
DESCRIPTION
SBPRID 
Pretensioner ID.  A unique number has to be used.
VARIABLE   
DESCRIPTION
SBPRTY 
Pretensioner type : 
EQ.1: pyrotechnic retractor with force limits, 
EQ.2: pre-loaded spring becomes active, 
EQ.3: lock spring removed, 
EQ.4: force versus time retractor. 
EQ.5: pyrotechnic  retractor  (old  type  in  version  950)  but  with
optional force limiter, LMTFRC. 
EQ.6: combination  of  types  4  and  5  as  described  in  the  notes
below. 
EQ.7: independent pretensioner/retractor. 
EQ.8: energy  versus  time  retractor  pretensioner  with  optional
force limiter, LMTFRC. 
EQ.9: energy versus time buckle or anchor pretensioner. 
SBSID1 
Sensor 1, see *ELEMENT_SEATBELT_SENSOR. 
SBSID2 
Sensor 2, see *ELEMENT_SEATBELT_SENSOR. 
SBSID3 
Sensor 3, see *ELEMENT_SEATBELT_SENSOR. 
SBSID4 
Sensor 4, see *ELEMENT_SEATBELT_SENSOR. 
SBRID 
Retractor  number  (SBPRTY = 1,  4,  5,  6,  7  or  8)  or  spring  element 
number (SBPRTY = 2, 3 or 9). 
TIME 
Time between sensor triggering and pretensioner acting. 
Load  curve  for  pretensioner  (Time  after  activation,  Pull-in) 
(SBPRTY = 1, 4, 5, 6, 7, 8 or 9). 
Optional  limiting  force  for  retractor  type  5  or  8.    If  zero,  this
option is ignored. 
PTLCID 
LMTFRC 
Activation: 
To activate the pretensioner, the following sequence of events must occur: 
1.  Any one of up to four sensors must be triggered. 
2.  Then a user-defined time delay occurs.
3.  Then the pretensioner acts. 
At least one sensor should be defined. 
Pretensioners  allow  modeling  of  seven  types  of  active  devices  which  tighten  the  belt 
during  the  initial  stages  of  a  crash.    Types  1  and  5  implement  a  pyrotechnic  device 
which spins the spool of a retractor, causing the belt to be reeled in.  The user defines a 
pull-in versus time curve which applies once the pretensioner activates.  Types 2 and 3 
implement preloaded springs or torsion bars which move the buckle when released. 
Types 2 and 3: 
The  pretensioner  is  associated  with  any  type  of  spring  element  including  rotational.  
Note that the preloaded spring, locking spring, and any restraints on the motion of the 
associated nodes are defined in the normal way; the action of the pretensioner is merely 
to cancel the force in one spring until (or after) it fires.  With the second type, the force 
in the spring element is canceled out until the pretensioner is activated.  In this case the 
spring in question is normally a stiff, linear spring which acts as a locking mechanism, 
preventing motion of the seat belt buckle relative to the vehicle.  A preloaded spring is 
defined in parallel with the locking spring.  This type avoids the problem of the buckle 
being free to ‘drift’ before the pretensioner is activated.  Types 4, 6, and 7, force types, 
are described below. 
Type 1: 
As of version 950 the type 1 (now type 5) pretensioner requires that the user provide a 
load  curve  tabulating  the  pull-in  of  the  pretensioner  as  a  function  of  time.    This 
pretensioner type interacts with the retractor, forcing it to pull in by the amount of belt 
indicated.  It works well, and does exactly what it says it will do, but it can be difficult 
to  use.    The  reason  for  this  is  that  it  has  no  regard  for  the  forces  being  exerted  on  the 
belt.    If  a  pull-in  of  20mm  is  specified  at  a  particular  time,  then  20mm  of  belt  will  be 
pulled in, even if this results in unrealistic forces in the seatbelt.  Furthermore, there was 
no  explicit  way  to  turn  this  pretensioner  off.    Once  defined,  it  overrode  the  retractor 
completely, and the amount of belt passing into or out of the retractor depended solely 
on the load curve specified. 
For the 970 release of LS-DYNA, the behavior of the type 1 pretensioner was  changed 
due to user feedback regarding these shortcomings.  Each retractor has a loading (and 
optional unloading) curve that describes the force on the belt element as a function of 
the  amount  of  belt  that  has  been  pulled  out  of  the  retractor  since  the  retractor  locked.  
The new type 1 pretensioner acts as a shift of this retractor load curve.  An example will 
make  this  clear.    Suppose  at  a  particular  time  that  5mm  of  belt  material  has  left  the 
retractor.  The retractor will respond with a force corresponding to 5mm pull-out on it's 
loading curve.  But suppose this retractor has a type 1 pretensioner defined, and at this
retractor
pull-out force
defined force
vs. time curve
retractor
lock time
Figure 17-17  Force versus time pretensioner.  At the intersection, the retractor
locks. 
Time
instant  of  time  the  pretensioner  specifies  a  pull-in  of  20mm.    The  retractor  will  then 
respond  with  a  force  that  corresponds  to  (5mm  +  20mm)  on  it's  loading  curve.    This 
results in a much larger force.  The effect can be that belt material will be pulled in, but 
unlike in the 950 version, there is no guarantee.  The benefit of this implementation is 
that  the  force  vs.    pull-in  load  curve  for  the  retractor  is  followed  and  no  unrealistic 
forces  are  generated.    Still,  it  may  be  difficult  to  produce  realistic  models  using  this 
option, so two new types of pretensioners have been added.  These are available in 970 
versions 1300 and later. 
Type 4: 
The type 4 pretensioner takes a force vs.  time curve, See Figure 17-17.  Each time step, 
the  retractor  computes  the  desired  force  without  regard  to  the  pretensioner.    If  the 
resulting  force  is  less  than  that  specified  by  the  pretensioner  load  curve,  then  the 
pretensioner value is used instead.  As time goes on, the pretensioner load curve should 
drop  below  the  forces  generated  by  the  retractor,  and  the  pretensioner  is  then 
essentially inactive.  This provides for good control of the actual forces, so no unrealistic 
values are generated.  The actual direction and amount of belt movement is unspecified, 
and will depend on the other forces being exerted on the belt.  This is suitable when the 
force the pretensioner exerts over time is known.
*ELEMENT_SEATBELT_PRETENSIONER 
The type 5 pretensioner is essentially the same as the old type 1 pretensioner, but with 
the addition of a force limiting value.  The pull-in is given as a function of time, and the 
belt is drawn into the retractor exactly as desired.  However, if at any point the forces 
generated  in  the  belt  exceed  the  pretensioner  force  limit,  then  the  pretensioner  is 
deactivated and the retractor takes over.  In order to prevent a large discontinuity in the 
force at this point, the loading curve for the retractor is shifted (in the abscissa) by the 
amount  required  to  put  the  current  (pull-out,  force)  on  the  load  curve.    For  example, 
suppose the current force is 1000, and the current pull-out is -10 (10mm of belt has been 
pulled IN by the pretensioner).  If the retractor would normally generate a force of 1000 
after 25mm of belt had been pulled OUT, then the load curve is shifted to the left by 35, 
and remains that way for the duration of the calculation.  So that at the current pull-in 
of  10,  it  will  generate  the  force  normally  associated  with  a  pull  out  of  25.    If  the  belt 
reaches a pull out of 5, the force will be as if it were pulled out 40 (5 + the shift of 35), 
and so on.  This option is included for those who liked the general behavior of the old 
type  1  pretensioner,  but  has  the  added  feature  of  the  force  limit  to  prevent  unrealistic 
behavior. 
Type 6: 
The  type  6  pretensioner  is  a  variation  of  the  type  4  pretensioner,  with  features  of  the 
type  5  pretensioner.    A  force  vs.    time  curve  is  input  and  the  pretensioner  force  is 
computed each cycle.  The retractor linked to this pretensioner should specify a positive 
value  for  PULL,  which  is  the  distance  the  belt  pulls  out  before  it  locks.    As  the 
pretensioner  pulls  the  belt  into  the  retractor,  the  amount  of  pull-in  is  tracked.    As  the 
pretensioner force decreases and drops below the belt tension, belt will begin to move 
back  out  of  the  retractor.    Once  PULL  amount  of  belt  has  moved  out  of  the  retractor 
(relative to the maximum pull in encountered), the retractor will lock.  At this time, the 
pretensioner  is  disabled,  and  the  retractor  force  curve  is  shifted  to  match  the  current 
belt tension.  This shifting is done just like the type 5 pretensioner.  It is important that a 
positive value of PULL be specified to prevent premature retractor locking which could 
occur due to small outward belt movements generated by noise in the simulation. 
Type 7: 
The  type  7  pretensioner  is  a  simple  combination  of  retractor  and  pretensioner.    It  is 
similar  to  the  type  6  except  for  the  following  changes:  when  the  retractor  locks,  the 
pretensioner is NOT disabled – it continues to exert force according to the force vs.  time 
curve until the end of the simulation.  (The force vs.  time curve should probably drop 
to 0 at some time.)  Furthermore, the retractor load curve is not shifted – the retractor 
begins  to  exert  force  according  to  the  force  vs.    pull-out  curve.    These  two  forces  are 
added  together  and  applied  to  the  belt.    Thus,  the  pretensioner  and  retractor  are 
essentially independent.
Type 8: 
The  type  8  pretensioner  is  a  variation  of  type  5  pretensioner.    The  pretension  energy, 
instead of pull-in for type 5, is given as a function of time.  This enables users to use a 
single pretensioner curve, PTLCID, for various sizes of dummies.  The energy could be 
yielded from the baseline test or simulation  by𝐸(𝑡) = ∫ 𝑓𝑑𝑝
, where f is the  force of the 
mouth element of the retractor and dp is the incremental pull-in. 
Type 9: 
The  type  9  pretensioner  is  designed  for  a  pretension-energy  based  buckle  or  anchor 
pretensioner.  The pretensioner is modeled as a spring element, SBRID.  One end of the 
spring  element  is  attached  to  the  vehicle.    For  a  buckle  pretensioner,  the  other  end  of 
SBRID  is  the  slip  ring  node,  SBRNID,  of  a  slip  ring  representing  the  buckle.    For  an 
anchor pretensioner, SBRID shares the other end with a belt element, see Figure
*ELEMENT_SEATBELT_RETRACTOR 
Purpose:  Define seat belt retractor.  See remarks below for seatbelt shell elements. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SBRID 
SBRNID 
SBID 
SID1 
SID2 
SID3 
SID4 
Type 
Default 
I 
0 
I 
0 
Remarks 
1,2 
  Card 2 
1 
2 
I 
0 
2 
3 
I 
0 
3 
4 
I 
0 
I 
0 
I 
0 
5 
6 
7 
8 
Variable 
TDEL 
PULL 
LLCID 
ULCID 
LFED 
Type 
F 
F 
Default 
0.0 
0.0 
Remarks 
F 
0.0 
I 
0 
4 
I 
0 
5 
  VARIABLE   
DESCRIPTION
SBRID 
Retractor ID.  A unique number has to be used. 
SBRNID 
Retractor node ID 
SBID 
SID1 
SID2 
SID3 
SID4 
Seat belt element ID 
Sensor ID 1 
Sensor ID 2 
Sensor ID 3 
Sensor ID 4
Before
Element 1
Element 1
Element 2
Element 4
Element 3
Element 2
After
Element 3
Element 4
Element 4
Element 4
All nodes within this area
are coincident
Figure 17-18.  Elements in a retractor. 
  VARIABLE   
DESCRIPTION
TDEL 
PULL 
Time delay after sensor triggers. 
Amount  of  pull-out  between  time  delay  ending  and  retractor
locking, a length value. 
LLCID 
Load curve for loading (Pull-out, Force), see Figure 17-18. 
ULCID 
Load curve for unloading (Pull-out, Force), see Figure 17-18. 
LFED 
Fed length, see explanation below. 
Remarks: 
1.  The  retractor  node  should  not  be  on  any  belt  elements.    The  element  defined 
should  have  one  node  coincident  with  the  retractor  node  but  should  not  be 
inside the retractor. 
2.  When  SBRNID < 0,  this  retractor  is  for  shell-type  seatbelt,  -SBRNID  is  the 
*SET_NODE  containing  RN1,  RN2,  …RN5.    SBID  is  then  *SET_SHELL_LIST.  
Note that the numbering of –SBRNID, SBID has to be consistent in the direction 
of  numbering.    For  example,  if  *SET_NODE  for  SBRNID  has  nodes  of  (RN1,
RN2, RN3, RN4, RN5) then *SET_SHELL_LIST for SBID should have elem.  of 
(RE1, RE2, RE3, RE4).  See Figure 17-16. 
3.  At least one sensor should be defined. 
4.  The  first  point  of  the  load  curve  should  be  (0,  Tmin).    Tmin  is  the  minimum 
tension.  All subsequent tension values should be greater than Tmin. 
5.  The  unloading  curve  should  start  at  zero  tension  and  increase  monotonically 
(i.e., no segments of negative or zero slope). 
Retractors  allow  belt  material  to  be  paid  out  into  a  belt  element.    Retractors 
operate in one of two regimes:  unlocked when the belt material is paid out, or 
reeled in under constant tension and locked when a user defined force-pullout 
relationship applies. 
The  retractor  is  initially  unlocked,  and  the  following  sequence  of  events  must 
occur for it to become locked: 
a)  Any  one  of  up  to  four  sensors  must  be  triggered.    (The  sensors  are  de-
scribed below.) 
b)  Then a user-defined time delay occurs. 
c)  Then a user-defined length of belt must be paid out (optional). 
d)  Then the retractor locks and once locked, it remains locked. 
In the unlocked regime, the retractor attempts to apply a constant tension to the 
belt.  This feature allows an initial tightening of the belt and takes up any slack 
whenever it occurs.  The tension value is taken from the first point on the force-
pullout load curve.  The maximum rate of pull out or pull in is given by 0.01 × 
fed  length  per  time  step.    Because  of  this,  the  constant  tension  value  is  not  al-
ways achieved. 
In  the  locked  regime,  a  user-defined  curve  describes  the  relationship  between 
the force in the attached element and the amount of belt material paid out.  If 
the tension in the belt subsequently relaxes, a different user-defined curve ap-
plies  for  unloading.    The  unloading  curve  is  followed  until  the  minimum  ten-
sion is reached. 
The curves are defined in terms of initial length of belt.  For example, if a belt is 
marked  at  10mm  intervals  and  then  wound  onto  a  retractor,  and  the  force  re-
quired  to  make  each  mark  emerge  from  the  (locked)  retractor  is  recorded,  the 
curves used for input would be as follows: 
0   Minimum tension (should be > zero)
10mm  Force to emergence of first mark 
20mm  Force to emergence of second mark 
⋮ 
Pyrotechnic pretensions may be defined which cause the retractor to pull in the 
belt at a predetermined rate.  This overrides the retractor force-pullout relation-
ship from the moment when the pretensioner activates. 
If desired, belt elements may be defined which are initially inside the retractor.  
These will emerge as belt material is paid out, and may return into the retractor 
if sufficient material is reeled in during unloading.  
Elements  e2,  e3  and  e4  are  initially  inside  the  retractor,  which  is  paying  out 
material into element e1.  When the retractor has fed Lcrit into e1, where 
Lcrit  = fed length - 1.1 × minimum length 
(minimum length defined on belt material input) 
(fed length defined on retractor input) 
Element  e2  emerges  with  an  unstretched  length  of  1.1  x  minimum  length;  the 
unstretched length of element e1 is reduced by the same amount.  The force and 
strain in e1 are unchanged; in e2, they are set equal to those in e1.  The retractor 
now pays out material into e2. 
If no elements are inside the retractor, e2 can continue to extend as more mate-
rial is fed into it. 
As  the  retractor  pulls in  the  belt  (for  example,  during  initial  tightening),  if  the 
unstretched  length  of  the  mouth  element  becomes  less  than  the  minimum 
length, the element is taken into the retractor. 
To  define  a  retractor,  the  user  enters  the  retractor  node,  the  ‘mouth’  element 
(into which belt material will be fed), e1 in Figure 17-18, up to 4 sensors which 
can trigger unlocking, a time delay, a payout delay (optional), load and unload 
curve numbers, and the fed length.   The retractor node is typically part of the 
vehicle  structure;  belt  elements  should  not  be  connected  to  this  node  directly, 
but  any  other  feature  can  be  attached  including  rigid  bodies.    The  mouth  ele-
ment should have a node coincident with the retractor but should not be inside 
the retractor.  The fed length would typically be set either to a typical element 
initial length, for the distance between painted marks on a real belt for compari-
sons  with  high  speed  film.    The  fed  length  should  be  at  least  three  times  the 
minimum length.
with weblockers
without weblockers
Figure 17-19.  Retractor force pull characteristics. 
Pullout
If  there  are  elements  initially  inside  the  retractor  (e2,  e3  and  e4  in  the  Figure) 
they should not be referred to on the retractor input, but the retractor should be 
identified  on  the  element  input  for  these  elements.    Their  nodes  should  all  be 
coincident with the retractor node and should not be restrained or constrained.  
Initial  slack  will  automatically  be  set  to  1.1  ×  minimum  length  for  these  ele-
ments; this overrides any user-defined value. 
Weblockers can be included within the retractor representation simply by enter-
ing a ‘locking up’ characteristic in the force pullout curve, see Figure 17-19.  The 
final section can be very steep (but must have a finite slope). 
6. 
In an event when only retractors are used in the model, be aware that the pull-
out is measured from the point when the retractor is locked.  If the belt has been 
pulled  IN  since  the  retractor  was  locked,  then  minimum  force  will  be  seen  in 
the  retractor  until  the  system  pays  out  enough  belt  to  get  back  to  the  point 
when locked 
If the behavior described in the above note undesirable then the type 6 preten-
sioner  model  is  recommended  for  the  seat  belt  system.    A  constant  force  vs.  
time load curve with a force equal to minimum tension fwill be defined, with a 
small  PULL  value  on  the  retractor.    With  this  set  up,  the  pretensioner  will  be 
active until the belt pulls all the way in, but as soon as the belt starts to move 
back out, the pretensioner will get disabled and the retractor will take over.
*ELEMENT 
Purpose:  Define seat belt sensor.  Four types are possible, see explanation below. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SBSID 
SBSTYP 
SBSFL 
Type 
Default 
I 
0 
I 
0 
I 
0 
Remarks 
Additional card for SBSTYP = 1. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID 
DOF 
ACC 
ATIME 
Type 
Default 
Remarks 
I 
0 
1 
I 
0 
F 
F 
0.0 
0.0 
Additional card for SBSTYP = 2. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SBRID 
PULRAT 
PULTIM 
Type 
Default 
I 
0 
F 
F 
0.0 
0.0 
Remarks
Additional card for SBSTYP = 3. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TIME 
Type 
F 
Default 
0.0 
Remarks 
Additional card for SBSTYP = 4. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID1 
NID2 
DMX 
DMN 
Type 
Default 
I 
0 
I 
0 
F 
F 
0.0 
0.0 
Remarks 
2 
2 
  VARIABLE   
DESCRIPTION
SBSID 
Sensor ID.  A unique number has to be used. 
SBSTYP 
Sensor type: 
EQ.1: acceleration of node, 
EQ.2: retractor pull-out rate, 
EQ.3: time, 
EQ.4: distance between nodes. 
SBSFL 
Sensor flag: 
EQ.0: sensor active during dynamic relaxation, 
EQ.1: sensor can be triggered during dynamic relaxation.
VARIABLE   
DESCRIPTION
NID 
DOF 
Node ID of sensor 
Degree of freedom: 
EQ.1: x, 
EQ.2: y, 
EQ.3: z. 
ACC 
Activating acceleration 
ATIME 
Time over which acceleration must be exceeded 
SBRID 
Retractor ID, see *ELEMENT_SEATBELT_RETRACTOR. 
PULRAT 
Rate of pull-out (length/time units) 
PULTIM 
Time over which rate of pull-out must be exceeded 
Time at which sensor triggers 
Node 1 ID 
Node 2 ID 
Maximum distance 
Minimum distance 
TIME 
NID1 
NID2 
DMX 
DMN 
Remarks: 
1.  Node  should  not  be  on  rigid  body,  velocity  boundary  condition,  or  other 
‘imposed motion’ feature. 
2.  Sensor  triggers  when  the  distance  between  the  two  nodes  is  d   >   dmax  or 
d  <  dmin.  Sensors are used to trigger locking of retractors and activate preten-
sioners.  Four types of sensors are available which trigger according to the fol-
lowing criteria: 
Type 1  When the magnitude of x-, y-, or z- acceleration of a given node has 
remained  above  a  given  level  continuously  for  a  given  time,  the 
sensor triggers.  This does not work with nodes on rigid bodies.
Type 2  When  the  rate  of  belt  payout  from  a  given  retractor  has  remained 
above  a  given  level  continuously  for  a  given  time,  the  sensor  trig-
gers. 
Type 3  The sensor triggers at a given time. 
Type 4  The sensor triggers when the distance between two nodes exceeds a 
given maximum or becomes less than a given minimum.  This type 
of sensor is intended for use with an explicit mass/spring represen-
tation of the sensor mechanism. 
By  default,  the  sensors  are  inactive  during  dynamic  relaxation.    This  allows 
initial tightening of the belt and positioning of the occupant on the seat without 
locking the retractor or firing any pretensioners.  However, a flag can be set in 
the  sensor  input  to  make  the  sensors  active  during  the  dynamic  relaxation 
phase.
*ELEMENT_SEATBELT_SLIPRING 
Purpose:  Define seat belt slip ring. 
Card 
1 
2 
3 
Variable 
SBSRID 
SBID1 
SBID2 
Type 
Default 
I 
0 
I 
0 
I 
0 
4 
FC 
F 
0.0 
5 
6 
7 
8 
SBRNID 
LTIME 
FCS 
ONID 
I 
0 
F 
F 
1020 
0.0 
I 
0 
Optional Card. 
  Card  2 
Variable 
Type 
1 
K 
F 
Default 
0.0 
  VARIABLE   
SBSRID 
SBID1 
SBID2 
FC 
2 
3 
4 
5 
6 
7 
8 
FUNCID 
DIRECT 
DC 
LCNFFD 
LCNFFS 
I 
0 
I 
0 
F 
0 
I 
0 
I 
0 
DESCRIPTION
Slip  ring  ID.    A  unique  number  has  to  be  used.    See  remarks
below for the treatment of slip rings for shell belt elements. 
Seat belt element 1 ID 
Seat belt element 2 ID 
Coulomb dynamic friction coefficient.  If less than zero, |FC| refers 
to  a  curve  which  defines  the  dynamic  friction  coefficient  as  a
function of time. 
SBRNID 
Slip ring node, NID 
LTIME 
Slip ring lockup time.  After this time no material is moved from
one  side  of  the  slip  ring  to  the  other.    This  option  is  not  active
during dynamic relaxation.
FCS 
*ELEMENT_SEATBELT_SLIPRING 
DESCRIPTION
Optional  Coulomb  static  friction  coefficient.    If  less  than  zero,
|FCS| refers to a curve which defines the static friction coefficient 
as a function of time. 
ONID 
Optional orientation node ID. 
K 
Optional  coefficient  for  determining  the  Coulomb  friction
coefficient related to angle alpha 
FUNCID 
Function ID to determine friction coefficient. 
DIRECT 
Direction of belt movement: 
EQ.0: 
if the belt can move along both directions. 
EQ.12:  if  the  belt  is  only  allowed  to  slip  along  the  direction
from SBID1 to SBID2 
EQ.21:  if  the  belt  is  only  allowed  to  slip  along  the  direction
from SBID2 to SBID 
DC 
Optional decay constant to allow a smooth transition between the
static and dynamic friction coefficients, i.e., 
𝜇𝑐 = FC + (FCS − FC)𝑒−DC×∣𝑣rel∣ 
LCNFFD 
LCNFFS 
Optional  curve  for  normal-force-dependent  Coulomb  dynamic 
friction  coefficient. 
friction 
coefficient  becomes  FC + 𝑓LCNFFD(𝐹𝑛),  where  𝑓LCNFFD(𝐹𝑛)  is  the 
function value of LCNFFD at contact force 𝐹𝑛. 
  When  defined, 
the  dynamic 
Optional  curve  for  normal-force-dependent  Coulomb  static 
friction  coefficient.    When  defined,  the  static  friction  coefficient
becomes  FCS + 𝑓LCNFFS(𝐹𝑛),  where  𝑓LCNFFS(𝐹𝑛)  is  the  function 
value of LCNFFS at contact force 𝐹𝑛.
Slipring Node
Orientation Node
Figure 17-20.  Orientation node. 
Remarks: 
When  SBRNID < 0,  this  slipring  is  for  shell-type  seatbelt,  -SBRNID  is  the  *SET_NODE 
containing SN1, SN2, …SN5.  SBID1 and SBID2 are then *SET_SHELL_LIST.  Note that 
the  numbering  of  -SBRNID,  SBID1  and  SBID2  has  to  be  consistent  in  the  direction  of 
numbering.    For  example  if,  *SET_NODE  for  SBRNID  has  nodes  of  (SN1,  SN2,  SN3, 
SN4,  SN5)  then  *SET_SHELL_LIST  for  SBID1  should  have  elem.    of  (SRE11,  SRE12, 
SRE13, SRE14) and *SET_SHELL_LIST for SBID2 should have elem.  of (SRE21, SRE22, 
SRE23, SRE24).  See Figure 17-20. 
Elements  1  and  2  should  share  a  node  which  is  coincident  with  the  slip  ring  node.  
Elements 1 and 2 should not be referenced in any other slipring definition.  The slip ring 
node should not be on any belt elements. 
Sliprings  allow  continuous  sliding  of  a  belt  through  a  sharp  change  of  angle.    Two 
elements  (1  &  2  in  Figure  17-21)  meet  at  the  slipring.    Node  B  in  the  belt  material
Slipring
Element 2
Element 1 
Element 3
Element 1
Element 2
Element 3 
Before 
After
Figure 17-21.  Elements passing through slipring. 
remains  attached  to  the  slipring  node,  but  belt  material  (in  the  form  of  unstretched 
length) is passed from element 1 to element 2 to achieve slip.  The amount of slip at each 
time step is calculated from the ratio of forces in elements 1 and 2.  The ratio of forces is 
determined  by  the  relative  angle  between  elements  1  and  2  and  the  coefficient  of 
friction,  FC.    The  tension  in  the  belts  are  taken  as  𝑇1  and  𝑇2,  where  𝑇2  is  on  the  high 
tension side and 𝑇1 is the force on the low tension side.  Thus, if 𝑇2 is sufficiently close 
to 𝑇1, no slip occurs; otherwise, slip is just sufficient to reduce the ratio 𝑇2/𝑇1 to 𝑒FC×𝜃, 
where 𝜃 is the wrap angle, see Figures 17-20 and 17-22  No slip occurs if both elements 
are slack.  The out-of-balance force at node B is reacted on the slip ring node; the motion 
of node B follows that of slip ring node. 
If, due to slip through the slip ring, the unstretched length of an element becomes less 
than  the  minimum  length  (as  entered  on  the  belt  material  card),  the  belt  is  remeshed 
locally:  the short element passes through the slip ring and reappears on the other side 
.  The new unstretched length of element 1 is 1.1 × minimum length.  
Force  and  strain  in  elements  2  and  3  are  unchanged;  force  and  strain  in  element  1  are 
now equal to those in element 2.  Subsequent slip will pass material from element 3 to 
element 1.  This process can continue with several elements passing in turn through the 
slip ring. 
To  define  a  slip  ring,  the  user  identifies  the  two  belt  elements  which  meet  at  the  slip 
ring,  the  friction  coefficient,  and  the  slip  ring  node.    The  two  elements  must  have  a 
common  node  coincident  with  the  slip  ring  node.    No  attempt  should  be  made  to 
restrain or constrain the common node for its motion will automatically be constrained
to  follow  the  slip  ring  node.    Typically,  the  slip  ring  node  is  part  of  the  vehicle  body 
structure and, therefore, belt elements should not be connected to this node directly, but 
any other feature can be attached, including rigid bodies. 
If K is undefined, the limiting force ratio is taken as 𝑒FC×𝜃.  If K is defined, the maximum 
force ratio is computed as  
𝑒FC×𝜃(1+K×𝛼2) 
where alpha is the angle shown in Figure 17-23.  The function is defined using the *DE-
FINE_FUNCTION  keyword  input.   This  function  is  a  function  of  three  variables,  and 
the ratio is given by evaluating 
𝑇2
𝑇1
= FUNC(FCT, 𝜃, 𝛼) 
where FCT is the instantaneous friction coefficient at time 𝑡, i.e.  it has the value of FC if 
the  belt  has  moved  in  the  last  time-step  and  the  value  of  FCS  if  the  belt  has  been 
stationary.    For  example,  the  default  behavior  can  be  obtained  using  the  function 
definition (assuming FCT has a value of 0.025 and the function ID is unity) 
*DEFINE_FUNCTION 
    1, 
f(fct,theta,alpha) = exp(0.025*theta) 
Behavior like default option can be obtained with (K=0.1): 
*DEFINE_FUNCTION 
  1, 
f(fct,theta,alpha) = exp(0.025*theta*(1.+0.1*alpha*alpha))
Figure 17-22.  Front view showing wrap angle. 
Figure 17-23.  Top view shows orientation of belt relative to axis.
*ELEMENT_SHELL_{OPTION} 
Available options include: 
<BLANK> 
THICKNESS  
BETA or MCID 
OFFSET 
DOF 
COMPOSITE 
COMPOSITE_LONG 
SHL4_TO_SHL8 
Stacking  of  options,  e.g.,  THICKNESS_OFFSET,  is  allowed  in  some  cases.    When 
combining  options  in  this  manner,  check  d3hsp  to  confirm  that  all  the  options  are 
acknowledged. 
Purpose:    Define  three,  four,  six,  and  eight  node  elements  including  3D  shells, 
membranes,  2D  plane  stress,  plane  strain,  and  axisymmetric  solids.    The  type  of  the 
element and its formulation is specified through the part ID  and the section 
ID .  Also, the thickness of each element can be specified when 
applicable on the element cards or else a default thickness value is used from the section 
definition. 
For orthotropic and anisotropic materials, a local material angle (variable BETA) can be 
defined which is cumulative with the integration point angles specified in *SECTION_-
SHELL,  *PART_COMPOSITE,  *ELEMENT_SHELL_COMPOSITE,  or  *ELEMENT_-
SHELL_COMPOSITE_LONG.    Alternatively,  the  material  coordinate  system  can  be 
defined as the projection of a local coordinate system, MCID, onto the shell.   
An  offset  option,  OFFSET,  is  available  for moving  the  shell  reference  surface  from  the 
nodal points that define the shell.   
The  COMPOSITE  or  COMPOSITE_LONG  option  allows  an  arbitrary  number  of 
integration  points  across  the  thickness  of  shells  sharing  the  same  part  ID.    This  is 
independent  of  thickness  defined  in  *SECTION_SHELL.      To  maintain  a  direct 
association  of  through-thickness  integration  point  numbers  with  physical  plies  in  the 
case where the number of plies varies from element to element, see Remark 12.
The option, SHL4_TO_SHL8, converts 3 node triangular and 4 node quadrilateral shell 
elements  to  6  node  triangular  and  8  node  quadrilateral  quadratic  shell  elements, 
respectively, by the addition of mid-side nodal points.  See Remark 9 below. 
For  the  shell  formulation  that  uses  additional  nodal  degrees-of-freedom,  the  option 
DOF is available to connect the nodes of the shell to corresponding scalar nodes.  Four 
scalar  nodes  are  required  for  element  type  25  to  model  the  thickness  changes  that 
require  2  additional  degrees-of-freedom  per  shell  node.    Defining  these  nodes  is 
optional, if left undefined, they will be automatically created. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
9 
Variable 
EID 
PID 
N1 
N2 
N3 
N4 
N5 
N6 
N7 
Type 
I 
I 
I 
I 
I 
I 
I 
Default 
none  none  none  none  none  none 
0 
I 
0 
I 
0 
10 
N8 
I 
0 
Remarks 
3 
3 
3 
3 
Thickness  Card.    Additional  card  for  THICKNESS,  BETA,  and  MCID  keyword 
options. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
THIC1 
THIC2 
THIC3 
THIC4 
BETA or MCID 
Type 
Default 
Remarks 
F 
0. 
1 
F 
0. 
F 
0. 
F 
0. 
F 
0.
Thickness  Card.    Additional  card  for  THICKNESS,  BETA,  and  MCID  keyword 
options, is only required if mid-side nodes are defined (N5-N8).. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
THIC5 
THIC6 
THIC7 
THIC8 
Type 
Default 
Remarks 
F 
0. 
6 
F 
0. 
F 
0. 
F 
0. 
. 
Offset Card.  Additional card for OFFSET keyword options. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
OFFSET 
Type 
Default 
Remarks 
F 
0.
Scalar Node Card.  Additional card for DOF keyword option. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
NS1 
NS2 
NS3 
NS4 
Type 
Default 
I 
I 
I 
I 
Remarks 
8 
8 
8 
8 
COMPOSITE Cards.  Additional set of cards for the COMPOSITE keyword option.  Set 
the  material  ID,  thickness,  and  material  angle  for  each  through-thickness  integration 
point of a composite shell are provided below (up to two integration points per card). 
The  integration  point  data  should  be  given  sequentially  starting  with  the  bottommost 
integration point.  The total number of integration points is determined by the number 
of  entries  on  these  cards.      The  thickness  of  each  shell  is  the  summation  of  the 
integration point thicknesses.  Define as many cards as needed. 
  Card 2 
1 
2 
Variable 
MID1 
THICK1 
Type 
I 
F 
3 
B1 
F 
4 
5 
6 
MID2 
THICK2 
I 
F 
8 
7 
B2 
F 
COMPOSITE_LONG  Cards.    Additional  set  of  cards  for  the  COMPOSITE_LONG 
keyword  option.    Set  the  material  ID,  thickness,  and  material  angle  for  each  through-
thickness  integration  point  of  a  composite  shell  are  provided  below  (one  integration 
point per card).  The integration point data should be given sequentially starting with 
the bottommost integration point.  The total number of integration points is determined 
by the number of entries on these cards.   The thickness of each shell is the summation 
of the integration point thicknesses.  Define as many cards as needed.  Column 4 must 
be left blank. 
  Card 2 
1 
2 
Variable 
MID1 
THICK1 
Type 
I 
F 
3 
B1 
F 
4 
5 
6 
7 
8 
PLYID1
VARIABLE   
DESCRIPTION
EID 
PID 
N1 
N2 
N3 
N4 
N5-N8 
THIC1 
THIC2 
THIC3 
THIC4 
BETA 
THIC5 
THIC6 
THIC7 
THIC8 
MCID 
Element  ID.    Chose  a  unique  number  with  respect  to  other
elements. 
Part ID, see *PART. 
Nodal point 1 
Nodal point 2 
Nodal point 3 
Nodal point 4 
Mid-side nodes for eight node shell 
Shell thickness at node 1 
Shell thickness at node 2 
Shell thickness at node 3 
Shell thickness at node 4 
Orthotropic material base offset angle .  The angle is given in degrees.  If blank the default is set 
to zero. 
Shell thickness at node 5 
Shell thickness at node 6 
Shell thickness at node 7 
Shell thickness at node 8 
Material coordinate system ID.  The a-axis of the base (or element-
level) material coordinate system  is the projection of the x-axis of 
coordinate  system  MCID  onto  the  surface  of  the  shell  element. 
The c-axis of the material coordinate system aligns with the shell
normal.      The  b-axis  is  taken  as  b = c  x  a.      Each  layer  in  the 
element  can  have  a  unique  material  orientation  by  defining  a
rotation angle for each layer as described in Remark 5.
n1
n1
n3
n2
*ELEMENT_SHELL 
n3
n3
Figure  17-24.    LS-DYNA  shell  elements.    Counterclockwise  node  numbering
determines the top surface. 
OFFSET 
The  offset  distance  from  the  plane  of  the  nodal  points  to  the
reference surface of the shell in the direction of the normal vector
to the shell. 
NS1 
NS2 
NS3 
NS4 
MID 
Scalar  node  1,  parameter  NDOF  on  the  *NODE_SCALAR  is 
normally set to 2.  If the thickness is constrained, set NDOF = 0. 
Scalar node 2 
Scalar node 3 
Scalar node 4 
Material ID of integration point 𝑖, see *MAT_… Section. 
THICK 
Thickness of integration point 𝑖. 
B 
Material angle of integration point 𝑖. 
PLYID 
Ply ID for integration point 𝑖 (for post-processing purposes). 
Remarks: 
1.  Default Thickness.  Default values in place of zero shell thicknesses are taken 
from the cross-section property definition of the PID, see *SECTION_SHELL. 
2.  Ordering.    Counterclockwise  node  numbering  determines  the  top  surface,  see 
Figure 17-24
3.  Coordinate  Systems.    Stresses  and  strain  output  in  the  binary  databases  are 
given  in  the  global  coordinate  system,  whereas  stress  resultants  are  output  in 
the local coordinate system for the shell element. 
4.  Convexity.  Interior angles must be less than 180 degrees. 
5.  Material  Orientation.    To  allow  the  orientation  of  orthotropic  and anisotropic 
materials  to  be  defined  for  each  shell  element,  a  BETA  angle  can  be  defined.  
This BETA angle is used with the AOPT parameter and associated data on the 
*MAT  card  to  determine  an  element  reference  direction  for  the  element.    The 
AOPT  data  defines  a  coordinate  system  and  the  BETA  angle  defines  a  subse-
quent  rotation  about  the  element  normal  to  determine  the  element  reference 
system.  For composite modeling, each layer in the element can have a unique 
material  direction  by defining  an  additional  rotation  angle  for the  layer,  using 
either the ICOMP and B𝑖 parameters on *SECTION_SHELL or the B𝑖 parameter 
on *PART_COMPOSITE.  The material direction for layer 𝑖 is then determined 
by a rotation angle, 𝜃𝑖 as shown in Figures 17-25 and 17-26.
i = β+β
Figure 17-25.  A multi-layer laminate can be defined.  The angle β
for the i’th lamina (integration point), see *SECTION_SHELL. 
i is defined
n4
n2
n3
n1
Figure 17-26.  Orientation of material directions (shown relative to the 1-2 side
as when AOPT = 0 in *MAT). 
6.  Activation  of  the  BETA  Field  and  Its  Interpretation.    To  activate  the  BETA 
field, either the BETA or THCKNESS keyword option must be used.  There is a 
difference  in  how  a  zero  value  or  empty field  is  interpreted.    When  the  BETA 
keyword  option  is  used,  a  zero  value  or  empty  BETA  field  will  override  the 
BETA  on  *MAT.    However,  when  the  THICKNESS  keyword  option  is  used,  a 
zero  value  or  empty  BETA  field  will  not  override  the  BETA  value  on  *MAT.  
Therefore,  to  input  BETA=0,  the  BETA  keyword  option  is  recommended.    If  a 
THIC value is omitted or input as  zero, the thickness will default to the value 
on the *SECTION_SHELL card.  If mid-side nodes are defined (N5-N8), then a 
second  line  of  thickness  values  will  be  read.    This  line  may  be  left  blank,  but 
cannot be omitted.  
7.  Offset  for  the  Reference  Surface.    The  parameter  OFFSET  gives  the  offset 
from the nodal points of the shell to the reference surface.  This option applies 
to  most  shell  formulations  excluding  two-dimensional  elements,  membrane 
elements, and quadratic shell elements.   Except for Mortar contacts, the refer-
ence  surface  offset  given  by  OFFSET  is  not  taken  into  account  in  the  contact
subroutines unless CNTCO is set to 1 in *CONTROL_SHELL.  For Mortar con-
tacts the OFFSET determines the location of the contact surface. 
8.  Scalar  Nodes.    The  scalar  nodes  specified  on  the  optional  card  refer  to  the 
scalar  nodes  defined  by  the  user  to  hold  additional  degrees  of  freedom  for 
shells with this capability.  Scalar nodes are used with shell element type 25 and 
26. 
9.  Automatic  Order  Increase.    The  option,  SHL4_TO_SHL8,  converts  3  node 
triangular  and  4  node  quadrilateral  shell  elements  to  6  node  triangular  and  8 
node  quadrilateral  quadratic  shell  elements,  respectively,  by  the  addition  of 
mid-side nodal points.  The user node ID’s for these generated nodes are offset 
after the largest user node ID defined in the input file.  When defining the *SEC-
TION_SHELL  keyword,  the  element  type  must  be  specified  as  either  23  or  24 
corresponding to quadratic quadrilateral and triangular shells, respectively.  
10.  Cohesive  Elements.    Cohesive  elements  (ELFORM=29,  46  or  47  on  *SEC-
TION_SHELL) may be defined with zero depth to connect surfaces with no gap 
between them, but must have nodes 1 and 2 on one surface and nodes 3 and 4 
on the other. 
11.  Contact  Thickness  when  using  *ELEMENT_SHELL_THICKNESS  in  MPP.  
When  using  MPP,  THEORY  =  1  in  *CONTROL_SHELL  has  special  meaning 
when  dealing  with  non-uniform-thickness  shells,  that  is,  it  serves  to  set  the 
nodal contact thickness equal to the average of the nodal thicknesses from the 
shells  sharing  that  node.    Thus  when  a  contact  surface  is  comprised  of  non-
uniform-thickness  shells,  THEORY  =  1  is  recommended  and  the  user  still  has 
the  option  of  setting  the  actual  shell  theory  using  ELFORM  in  *SECTION_-
SHELL. 
12.  Assignment  of  Zero  Thickness  to  Integration  Points.    The  ability  to  assign 
zero- thickness integration points in the stacking sequence allows the number of 
integration points to remain constant even as the number of physical plies var-
ies  from  element  to  element  and  eases  post-processing  since  a  particular  inte-
gration  point  corresponds  to  a  physical  ply.    Such  a  capability  is  important 
when  one  or  more  of  the  physical  plies  are  not  continuous  across  a  part.    To 
represent a missing ply in *ELEMENT_SHELL_COMPOSITE, set THICKi to 0.0 
for the corresponding integration point and additionally, either set MID=-1 or, 
if the LONG option is used, set PLYID to any nonzero value.  
When  postprocessing  the  results  using  LS-PrePost  version  4.5,  read  both  the 
keyword deck and d3plot database into the code and then select    Option > N/A 
gray  fringe.    Then,  when  viewing  fringe  plots  for  a  particular  integration  point 
(FriComp > IPt > intpt#),  the  element  will  be  grayed  out  if  the  selected  integra-
tion point is missing (or has zero thickness) in that element.
*ELEMENT_SHELL_NURBS_PATCH 
Purpose:    Define  a  NURBS-surface  element  (patch)  based  on  a  rectangular  grid  of 
control points.  This grid consists of NPR*NPS control points, where NPR and NPS are 
the  number  of  control  points  in  local  r-  and  s-direction,  respectively.    The  necessary 
shape functions are defined through two knot-vectors: 
1.  Knot-Vector in r-direction with length NPR + PR + 1 and 
2.  Knot-Vector in s-direction with length NPS + PS + 1 
There is no limit on the size of the underlying grid to define a NURBS-surface element, 
so  the  total  number  of  necessary  Keyword-cards  depends  on  the  parameters  given  in 
the first two cards and is given by 
# of cards  = 2 + ⌈
NPR + PR + 1
⌉ + ⌈
NPS + PS + 1
⌉ + NPS × ⌈
NPR
⌉, 
where ⌈𝑥⌉ = ceil(𝑥).  (NOTE: the last term in the sum  is doubled if WFL = 1, indicating 
that the weights are user-specified). 
An example partial keyword deck using this card is given in Figure 17-28. 
  Card 1 
1 
2 
3 
Variable 
NPID 
PID 
NPR 
Type 
I 
I 
I 
4 
PR 
I 
5 
NPS 
I 
6 
PS 
I 
7 
8 
Default 
none 
none 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
Variable 
WFL 
FORM 
INT 
NISR 
NISS 
IMASS 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
I 
PR 
PS 
I 
0 
8 
7 
NL 
I 
0 
Remarks 
Figure 
17-28 
Figure 
17-28
Knot Vector Cards (for r-direction).  The knot-vector in local r-direction with length 
NPR +PR + 1  is  given  below  (up  to  eight  values  per  card)  requiring  a  total  of 
Ceil[ (NPR +PR + 1)/8 ] cards. 
  Cards A 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RK1 
RK2 
RK3 
RK4 
RK5 
RK6 
RK7 
RK8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Knot Vector Cards (for s-direction).  The knot-vector in local s-direction with length 
NPS +PS + 1  is  given  below  (up  to  eight  values  per  card)  requiring  a  total  of 
Ceil[ (NPS +PS + 1)/8 ] cards. 
 Cards B 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SK1 
SK2 
SK3 
SK4 
SK5 
SK6 
SK7 
SK8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Connectivity Cards.  The connectivity of the control grid is a two dimensional table of 
NPS  rows  and  NPR  columns.    This  data  fills  NPS  sets  (one  set  for  each  row)  of  NPR 
points  tightly  packed  into  Ceil( NPR/8 )  Connectivity  Cards  (format  C),  for  a  total  of 
NPS × Ceil( NPR/8 ) cards. 
 Cards C 
Variable 
1 
N1 
Type 
I 
2 
N2 
I 
3 
N3 
I 
4 
N4 
I 
5 
N5 
I 
6 
N6 
I 
7 
N7 
I 
8 
N8 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none
Weight  cards.    Additional  cards  for  WFL ≠ 0.    Set  a  weight  for  each  control  point. 
These cards have an ordering identical to the Connectivity Cards (cards “C”). 
 Cards D 
1 
Variable 
W1 
2 
W2 
3 
W3 
4 
W4 
5 
W5 
6 
W6 
7 
W7 
8 
W8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Trimming Loop cards.  Additional cards for NL.gt.0.  
For every trimming loop (NL) define a set of Cards (E1 and E2). 
Cards E1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NLE 
Type 
I 
Trimming Loop cards.  
Define NLE (Number of loop edges) edges (Ei).  Use as many cards (E2) as necessary 
Cards E2 
Variable 
1 
E1 
Type 
I 
2 
E2 
I 
3 
E3 
I 
4 
E4 
I 
5 
E5 
I 
6 
E6 
I 
7 
E7 
I 
8 
E8 
I 
 VARIABLE  
DESCRIPTION 
NPID 
Nurbs-Patch Element ID.  A unique number has to be chosen 
PID 
NPR 
PR 
Part ID, see *PART. 
Number of control points in local r-direction. 
Order of polynomial of univariate nurbs basis functions in local 
r-direction.
NPS 
PS 
Number of control points in local s-direction. 
Order of polynomial of univariate nurbs basis functions in local 
s-direction. 
WFL 
Flag for weighting factors of the control points 
EQ.0:  all  weights  at  the  control  points  are  set  to  1.0  (B-spline 
basis) and no optional cards D are allowed 
NE.0:  the  weights  at  the  control  points  are  defined  in  optional
cards D which must be defined after cards C. 
FORM 
Shell formulation to be used 
EQ.0: 
EQ.1: 
shear deformable shell theory with rotational DOFs 
shear deformable shell theory without rotational DOFs 
EQ.2: 
thin shell theory without rotational DOFs 
EQ.-4/4:  combination of FORM = 0 and FORM = 1 
INT 
In-plane numerical integration rule. 
EQ.0:  uniformly reduced Gauss integration, NIP = PR × PS. 
EQ.1:  full Gauss integration, NIP = (PR+1) × (PS+1). 
EQ.2:  reduced,  patch-wise  integration  rule  for  C1-continuous 
quadratic NURBS 
NISR 
NISS 
Number  of  (automatically  created)  Interpolation  Shell  elements  in
local  r-direction  per  created  Nurbs-element  for  visualization 
(postprocessing) and contact . 
Number  of  (automatically  created)  Interpolation  Shell  elements  in
local  s-direction  per  created  Nurbs-element  for  visualization 
(postprocessing) and contact . 
IMASS 
Option for lumping of mass matrix: 
EQ.0:  row sum  
EQ.1:  diagonal weighting. 
NL 
Number of trimming loops  
EQ.0:  no trimming loops – standard untrimmed NURBS  
GT.0:  trimmed NURBS with NL trimming loops
Values  of  the  univariate  knot  vector  in  local  r-direction  defined  in 
cards A. 
Values  of  the  univariate  knot  vector  in  local  s-direction  defined  in 
cards B. 
Control  points  i  (defined  via  *NODE)  to  define  the  control  grid  in
cards C.  
LT.0 (FORM = 4/-4):  control  point  with  rotational  DOFs 
(6 
DOFs/control point, see remark 3) 
Weighting factors of the control point i defined in cards D. 
Number of loop edges to define trimming loop in cards E1 (NL.gt.0)
Edge  (Curve)  ID  defining  this  edge  –  use  *DEFINE_CURVE  with 
DATTYP = 6 
RKi 
SKi 
Ni 
Wi 
NLE 
Ei 
Remarks: 
1.  The  thickness  of  the  shell  is  defined  in  *SECTION_SHELL  (referenced  via 
*PART). 
2.  ELFORM = 201 has to be used in *SECTION_SHELL. 
3.  FORM = 4  allows  the  mixture  of  control  points  with  and  without  rotational 
DOFs.    This  might  be  useful  at  the  boundaries  of  Nurbs-patches  where  the 
continuity usually drops to C0 and rotational DOFs are necessary.  To indicate 
control  points  with  rotational  DOFs  (6  DOFs/control  point), the  node  number 
of the corresponding control point has to be set as the negative node ID in the 
connectivity  cards  C.    Positive  node  IDs  indicate  control  points  without  rota-
tional DOFs (3 DOFs/control point). 
If FORM = -4 is used, the control points at the patch boundary are automatically 
treated with rotational DOFs without the need to specify them explicitly in the 
connectivity cards C.  This might be sufficient in many cases.  
4.  The  post-processing  and  the  treatment  of  contact  boundary  conditions  are 
presently  dealt  with  interpolation  elements,  defined  via  interpolation  nodes.  
These  nodes  and  elements  are  automatically  created,  where  NISR  and  NISS 
indicate the number of interpolation elements to be created per NURBS-element 
in the local r- and s-direction, respectively .
individual  edges 
5.  Trimmed  NURBS-patches  can  be  analyzed  by  defining  trimming  loops 
(NL.gt.0) in Card 2.  For each trimming loop to be defined, a set of cards E (E1 
and E2), specifying the number of edges together with the edge (curve) IDs of 
is  defined  via 
the 
*DEFINE_CURVE  using  DATTYP = 6.    The  order  of  the  edges  as  well  as  the 
order  of  the  vertex  nodes  in  *DEFINE_CURVE  need  to  be  in  order,  to  define 
either a clockwise or a counter-clockwise orientation of the trimming loop.  The 
orientation of the trimming loop is essential in defining, which part of the patch 
shall  be  trimmed  away.    Travelling  along  the  trimming  loop,  the  right-hand 
side of the trimming line will be cut away. 
is  necessary. 
  One  edge 
itself 
6.  The trimming loops need to be defined in the parametric (local) rs-space of the 
NURBS-patch with r/s in [0,1].  The last and the first vertex node of consecutive 
edges need to coincide.
Nurbs-Surface (physical space)
38
37
36
27
26
39
28
29
35
25
17
16
18
19
34
24
15
23
14
33
32
31
22
13
21
12
11
Nurbs-Surface (parameter space)
-
)
-
(
]
,
,
,
,
,
,
[
:
-
B-spline basis functions (r-direction)
r-knot: [0,0,0,1,2,3,4,5,6,7,7,7]
Control Points (*NODE)
Control Net
(*ELEMENT_SHELL_NURBS_PATCH)
Connectivity of
Nurbs-Element (automatic)
Nurbs-Element (automatic)
Interpolation Node (automatic)
Interpolation Element (automatic)
Interpolation Elements
(postprocessing/contact/BC)
NISR=2 / NISS=2
Figure 17-27.  Illustration of example input deck from Figure 17-28.
*ELEMENT_SHELL_NURBS_PATCH
$ Card 1
$---+-NPID----+--PID----+--NPR----+---PR----+--NPS----+---PS----+----7----+----8
2 
11 
12 
4 
9 
$ Card 2
$---+--WFL----+-FORM----+--INT----+-NISR----+-NISS----+IMASS----+----7----+----8
2 
1 
0 
1 
2 
$ Cards A
$rk-+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8
5.0
2.0 
3.0 
4.0 
0.0 
6.0 
0.0 
7.0 
0.0 
7.0 
1.0 
7.0
$ Cards B
$sk-+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8
0.0 
0.0 
0.0 
1.0 
2.0 
2.0 
2.0
$ Cards C
$net+---N1----+---N2----+---N3----+---N4----+---N5----+---N6----+---N7----+---N8
4 
7 
3 
5 
2 
6 
12 
22 
32 
13 
23 
33 
14 
24 
34 
15 
25 
35 
16 
26 
36 
17 
27 
37 
18
28
38
$ Cards D (optional if WFL.ne.0)
$wgt+---W1----+---W2----+---W3----+---W4----+---W5----+---W6----+---W7----+---W8
0.8
0.7 
0.8 
0.9 
0.8 
0.9 
0.7 
0.7 
0.6 
0.9 
0.6 
0.5 
0.8 
0.5 
0.4 
0.7 
0.6 
0.5 
0.8 
0.7 
0.6 
0.9 
0.6 
0.5 
0.7 
0.7
0.6
0.8
1 
11 
19
21 
29
31 
39
1.0 
1.0
0.8 
0.8
0.7 
0.7
1.0 
1.0
Figure  17-28.    Example  of  a  bi-quadratic  *ELEMENT_SHELL_NURBS_-
PATCH keyword definition.  See Figure 17-27 below.
*ELEMENT_SHELL_SOURCE_SINK 
Purpose:    Define  a  strip  of  shell  elements  of  a  single  part  ID  to  simulate  a  continuous 
forming  operation.    This  option  requires  logical  regular  meshing  of  rectangular 
elements,  which  implies  that  the  number  of  nodal  points  across  the  strip  is  constant 
along  the  length.      Elements  are  created  at  the  source  and  disappear  at  the  sink.    The 
advantage of this approach is that it is not necessary to define an enormous number of 
elements to simulate a continuous forming operation.   Currently, only one source-sink 
definition  is  allowed.    The  boundary  conditions  at  the  source  are  discrete  nodal  point 
forces to keep the work piece in tension.  At the sink, displacement boundary conditions 
are applied. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSSR 
NSSK 
PID 
Type 
I 
I 
I 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION
NSSR 
NSSK 
Node  set  at  source.    Provide  an  ordered  set  of  nodes  between 
corner nodes, which include the corner nodes. 
Node set at sink.  Provide an ordered set of nodes between corner
nodes, which include the corner nodes. 
PID 
Part ID of work piece.
*ELEMENT_SOLID_{OPTION} 
Available options include: 
<BLANK> 
ORTHO 
DOF 
TET4TOTET10 
H20 
H8TOH20 
H27 
H8TOH27 
Purpose:  Define three-dimensional solid elements including 4 noded tetrahedrons and 
8-noded  hexahedrons.    The  type  of  solid  element  and  its  formulation  is  specified 
through the part ID  and the section ID .  
Also, a local coordinate system for orthotropic and anisotropic materials can be defined 
by using the ORTHO option.  If extra degrees of freedom are needed, the DOF option 
should  be  used.    The  option  TET4TOTET10  converts  4  node  tetrahedrons  to  10  node 
tetrahedrons,  and  H8TOH20/H8TOH27  converts  8-node  hexahedrons  to  20-node/27-
node hexahedrons.  See Remark 1. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
EID 
PID 
Type 
I 
I 
Default 
none  none 
Remarks
Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
N1 
N2 
N3 
N4 
N5 
N6 
N7 
N8 
N9 
N10 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none  none  none  none  none  none  none  none  none  none 
20 Node Element Card.  Additional card for the 20 option. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
N11 
N12 
N13 
N14 
N15 
N16 
N17 
N18 
N19 
N20 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none  none  none  none  none  none  none  none  none  none 
27 Node Element Card.  Additional card for the 27 option. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
N11 
N12 
N13 
N14 
N15 
N16 
N17 
N18 
N19 
N20 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none  none  none  none  none  none  none  none  none  none 
Variable 
N21 
N22 
N23 
N24 
N25 
N26 
N27 
Type 
I 
I 
I 
I 
I 
I 
I 
Default 
none  none  none  none  none  none  none
Orthotropic Card 1.  Additional card for ORTHO keyword option. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
A1 or BETA 
Type 
Default 
F 
0. 
Remarks 
5, 7 
A2 
F 
0. 
A3 
F 
0. 
Orthotropic Card 2.  Second additional card for ORTHO keyword option. 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
D1 
Type 
Default 
Remarks 
F 
0. 
5 
D2 
F 
0. 
D3 
F 
0. 
Scalar Node Card.  Additional cards for DOF keyword option.  This input ends at the 
next keyword “*” card. 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
NS1 
NS2 
NS3 
NS4 
NS5 
NS6 
NS7 
NS8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none  none  none  none  none  none  none  none 
  VARIABLE   
DESCRIPTION
EID 
Element ID.  A unique number has to be chosen.
VARIABLE   
DESCRIPTION
PID 
Part ID, see *PART. 
N1 
N2 
N3 
⋮ 
Nodal point 1 
Nodal point 2 
Nodal point 3 
            ⋮ 
N27 
Nodal point 27 
A1 or BETA 
𝑥-component  of  local  material  direction  a,  or  else  rotation  angle 
BETA in degrees .
10
15
16
20
17
14
19
18
13
11
12
10
4-node n1, n2, n3, n4, n4, n4, n4, n4
6-node n1, n2, n3, n4, n5, n5, n6 ,n6
Figure  17-29.    Four,  six,  eight,  ten,  and  twenty  node  solid  elements.    For
the  hexahedral  and  pentahedral  shapes,  nodes  1-4  are  on  the  bottom
surface. 
  VARIABLE   
DESCRIPTION
A2 
A3 
D1 
D2 
𝑦-component of local material direction 𝐚. 
𝑧-component of local material direction 𝐚. 
𝑥-component of vector in the plane of the material vectors 𝐚 and 
𝐛. 
𝑦-component of vector in the plane of the material vectors 𝐚 and 
𝐛.
VARIABLE   
DESCRIPTION
𝑧-component  of  vector in  the  plane  of  the  material  vectors 𝐚  and 
𝐛. 
Scalar node 1.  See Remark 8. 
Scalar node 2 
Scalar node 3 
Scalar node 4 
Scalar node 5 
Scalar node 6 
Scalar node 7 
Scalar node 8 
D3 
NS1 
NS2 
NS3 
NS4 
NS5 
NS6 
NS7 
NS8 
Remarks: 
1.  Automatic  Node  Generation.    The  option  TET4TOTET10  automatically 
converts  4  node  tetrahedron  solids  to  10  node  quadratic  tetrahedron  solids.  
Additional  mid-side  nodes  are  created  which  are  shared  by  all  tetrahedron 
elements that contain  the edge.  The  user node ID’s for these generated nodes 
are offset after the largest user node ID defined in the input file.  When defining 
the *SECTION_SOLID keyword, the element type must be specified as either 16 
or 17 which are the 10-noded tetrahedrons in LS-DYNA.  Mid-side nodes creat-
ed  as  a  result  of  TET4TOTET10  will  not  be  automatically  added  to  node  sets 
that include the nodes of the original tetrahedron.  So, for example, if the tetra-
hedrons are to have an initial velocity, velocity initialization by part ID or part 
set  ID  using  *INITIAL_VELOCITY_GENERATION  is  necessary  as  opposed  to 
velocity  initialization  by  node  set  ID  using  *INITIAL_VELOCITY.    The  option 
H8TOH20/H8TOH27 provides the same functionality for converting 8-node to 
20-node/27-node elements. 
2.  Node  Numbering.    Four,  six,  and  eight  node  elements  are  shown  in  Figure 
17-29  where  the  ordering  of  the  nodal  points  is  shown.    27-node  elements  are 
shown in Figure 0-3.  This ordering must be followed or code termination with 
occur  during  the  initialization  phase  with  a  negative  volume  message.    The 
input  of  nodes  on  the  element  cards  for  the  tetrahedron  and  pentahedron  ele-
ments is given by: 
4-noded tetrahedron 
N1, N2, N3, N4, N4, N4, N4, N4, 0, 0
c is orthogonal
to the a,d plane
c = a × d 
a,d are input.
The computed
axes do not
depend on the
element.
b = c × a 
b is orthogonal
to the c,a plane
Figure  17-30.  Two vectors a and d are defined and the triad is computed and
stored. 
6-noded pentahedron 
N1, N2, N3, N4, N5, N5, N6, N6, 0, 0 
3.  Degenerate  Solids. 
  If  hexahedrons  are  mixed  with  tetrahedrons  and 
pentahedrons in the input under the same part ID, degenerate tetrahedrons and 
pentahedrons are used.  One problem with degenerate elements is related to an 
uneven mass distribution (node 4 of the tetrahedron has five times the mass of 
nodes 1-3) which can make these elements somewhat unstable with the default 
time step size.  By using the control flag under the keyword, *CONTROL_SOL-
ID, automatic sorting can be invoked to treat the degenerate elements as type 10 
and type 15 tetrahedron and pentahedron elements, respectively. 
4.  Obsolete Card Format.  For elements with 4-8 nodes the cards in the format of 
LS-DYNA  versions  940-970  are  still  supported.    The  older  format  does  not  in-
clude Card 2. 
Obsolete Element Solid Card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
9 
Variable 
EID 
PID 
N1 
N2 
N3 
N4 
N5 
N6 
N7 
10 
N8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
I 
I 
5.  Local  Directions.    For  the  orthotropic  and  anisotropic  material  models  the 
local directions may be defined on the second card following the element con-
nectivity definition.  The local directions are then computed from the two vec-
tors such that : 
𝐜 = 𝐚 × 𝐝  and 𝐛 = 𝐜 × 𝐚.
These vectors are internally normalized within LS-DYNA.  If the material mod-
el uses AOPT = 3, the 𝑎 and 𝑏 axes will be rotated about the 𝑐 axis by the BETA 
angle on the material card. 
6.  Stress  Output  Coordinates.    Stress  output  for  solid  elements  is  in  the  global 
coordinate system by default. 
7. 
Interpretation of A1 Field.  If vector 𝐝 is input as a zero length vector, then A1 
is  interpreted  as  an  offset  rotation  angle  BETA  in  degrees  which  describes  a 
rotation about the 𝐜-axis of the 𝐚-𝐛-𝐜 coordinate system that is defined by AOPT 
and associated parameters on the *MAT input.  This BETA angle applies to all 
values of AOPT, and it overrides the BETA angle on the *MAT card in the case 
of AOPT=3. 
7 
14 
15 
8.  Optional  “Scalar”  Nodes.    The  scalar  nodes  specified  on  the  optional  card 
refer to extra nodes used by certain features (usual user defined) to store addi-
tional degrees of freedom.
16 
26 
8 
13
17
18
19 
3 
10 
11 
12 
0 
4 
22 
23
24
27 
21
25 
Figure  17-3.  27-node solid element.
*ELEMENT_SOLID_NURBS_PATCH 
Purpose:    Define  a  NURBS-block  element  (patch)  based  on  a  cuboid  grid  of  control 
points.  This grid consists of NPR*NPS*NPT  control points, where NPR, NPS and NPT 
are  the  number  of  control  points  in  local  r-,  s-  and  t-direction,  respectively.    The 
necessary shape functions are defined through three knot-vectors: 
1.  Knot-Vector in r-direction with length NPR + PR + 1 and 
2.  Knot-Vector in s-direction with length NPS + PS + 1 and 
3.  Knot-Vector in t-direction with length NPT + PT + 1 and 
There is no limit on the size of the underlying grid to define a NURBS-block element, so 
the total number of necessary Keyword-cards depends on the parameters given in the 
first two cards and is given by 
# of cards  = 2 + ⌈
NPR + PR + 1
⌉ + ⌈
NPS + PS + 1
⌉ + ⌈
NPT + PT + 1
⌉ + NPT × NPS
× ⌈
NPR
⌉, 
where ⌈𝑥⌉ = ceil(𝑥).  (NOTE: the last term in the sum  is doubled if WFL = 1, indicating 
that the weights are user-specified). 
An example partial keyword deck using this card is given at the end. 
  Card 1 
1 
2 
3 
Variable 
NPID 
PID 
NPR 
Type 
I 
I 
I 
4 
PR 
I 
5 
NPS 
I 
6 
PS 
I 
7 
NPT 
I 
8 
PT 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none
Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
WFL 
NISR 
NISS 
NIST 
IMASS 
Type 
Default 
I 
0 
Remarks 
I 
I 
I 
PR 
PS 
PT 
I 
0 
Knott Vector Cards (for r-direction).  The knot-vector in local r-direction with length 
NPR +PR + 1  is  given  below  (up  to  eight  values  per  card)  requiring  a  total  of 
Ceil[ (NPR +PR + 1)/8 ] cards. 
  Cards A 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RK1 
RK2 
RK3 
RK4 
RK5 
RK6 
RK7 
RK8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Knott Vector Cards (for s-direction).  The knot-vector in local s-direction with length 
NPS +PS + 1  is  given  below  (up  to  eight  values  per  card)  requiring  a  total  of 
Ceil[ (NPS +PS + 1)/8 ] cards. 
 Cards B 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SK1 
SK2 
SK3 
SK4 
SK5 
SK6 
SK7 
SK8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none
Knott Vector Cards (for t-direction).  The knot-vector in local t-direction with length 
NPT +PT + 1  is  given  below  (up  to  eight  values  per  card)  requiring  a  total  of 
Ceil[ (NPT+PT + 1)/8 ] cards. 
 Cards C 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TK1 
TK2 
TK3 
TK4 
TK5 
TK6 
TK7 
TK8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Connectivity Cards.  The connectivity of the control grid is a two dimensional table of 
NPT ×  NPS  rows  and  NPR  columns.    This  data  fills  NPT ×  NPS  sets  (one  set  for  each 
row)  of  NPR  points  tightly  packed  into  Ceil( NPR/8 )  Connectivity  Cards  (format  C), 
for a total of NPT × NPS × Ceil( NPR/8 ) cards. 
 Cards D 
Variable 
1 
N1 
Type 
I 
2 
N2 
I 
3 
N3 
I 
4 
N4 
I 
5 
N5 
I 
6 
N6 
I 
7 
N7 
I 
8 
N8 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Weight  cards.    Additional  cards  for  WFL ≠ 0.    Set  a  weight  for  each  control  point. 
These cards have an ordering identical to the Connectivity Cards (cards “D”). 
  Cards E 
1 
Variable 
W1 
2 
W2 
3 
W3 
4 
W4 
5 
W5 
6 
W6 
7 
W7 
8 
W8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
 VARIABLE  
DESCRIPTION 
NPID 
Nurbs-Patch Element ID.  A unique number has to be chosen
PID 
NPR 
PR 
NPS 
PS 
NPT 
PT 
Part ID, see *PART. 
Number of control points in local r-direction. 
Order of polynomial of univariate nurbs basis functions in local 
r-direction. 
Number of control points in local s-direction. 
Order of polynomial of univariate nurbs basis functions in local 
s-direction. 
Number of control points in local t-direction. 
Order of polynomial of univariate nurbs basis functions in local 
t-direction. 
WFL 
Flag for weighting factors of the control points 
EQ.0: all  weights  at  the  control  points  are  set  to  1.0  (B-spline 
basis) and no optional cards E are allowed 
NE.0:  the  weights  at  the  control  points  are  defined  in  optional 
cards E which must be defined after cards D. 
Number  of  (automatically  created)  Interpolation  Solid  elements  in
local  r-direction  per  created  Nurbs-element  for  visualization 
(postprocessing) and contact. 
Number  of  (automatically  created)  Interpolation  Solid  elements  in
local  s-direction  per  created  Nurbs-element  for  visualization 
(postprocessing) and contact. 
Number  of  (automatically  created)  Interpolation  Solid  elements  in
local  t-direction  per  created  Nurbs-element  for  visualization 
(postprocessing) and contact. 
NISR 
NISS 
NIST 
IMASS 
Option for lumping of mass matrix: 
EQ.0: row sum  
EQ.1: diagonal weighting. 
RKi 
SKi 
Values  of  the  univariate  knot  vector  in  local  r-direction  defined  in 
cards A. 
Values  of  the  univariate  knot  vector  in  local  s-direction  defined  in 
cards B.
Values  of  the  univariate  knot  vector  in  local  t-direction  defined  in 
cards C. 
Control  points  i  (defined  via  *NODE)  to  define  the  control  grid  in
cards D.  
Weighting factors of the control point i defined in cards E. 
TKi 
Ni 
Wi 
Remarks: 
1.  ELFORM = 201 has to be used in *SECTION_SOLD. 
2.  The  post-processing  and  the  treatment  of  contact  boundary  conditions  are 
presently  dealt  with  interpolation  elements,  defined  via  interpolation  nodes.  
These  nodes  and  elements  are  automatically  created,  where  NISR,  NISS  and 
NIST indicate the number of interpolation elements to be created per NURBS-
element in the local r-, s- and t-direction, respectively. 
3.  An input deck can be shown as follows. 
Example: 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
$ An Isogeometric Solid NURBS Example : 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
*SECTION_SOLID 
$#   secid    elform      
         1       201              
*ELEMENT_SOLID_NURBS_PATCH 
$CARD 1 
$#   npeid       pid       npr        pr       nps        ps       npt        pt 
         1         1         3         2         6         2         3         2 
$CARD 2 
$#     wfl      nisr      niss      nist     imass 
         0         2         2         2         0 
$CARD A 
$#     rk1       rk2       rk3       rk4       rk5       rk6       rk7       rk8 
       0.0       0.0       0.0       1.0       1.0       1.0  
$CARD B 
       0.0       0.0       0.0      0.25       0.5      0.75       1.0       1.0 
       1.0 
$CARD C 
       0.0       0.0       0.0       1.0       1.0       1.0  
$CARD D 
      1001      1002      1003 
       … 
      1052      1053      1054    
$CARD E (Optional if wfl .eq.  0)
*ELEMENT_SPH 
Purpose:  Define a lumped mass element assigned to a nodal point. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
NID 
PID 
MASS 
Type 
I 
I 
Default 
none  none 
Remarks 
F 
0. 
1 
  VARIABLE   
DESCRIPTION
Node ID and Element ID are the same for the SPH option. 
Part ID to which this node (element) belongs. 
GT.0: Mass value 
LT.0:  Volume.  The absolute value will be used as volume.  The
density  (rho)  will  be  retrieved  from  the  material  card
defined  in  PID.    SPH  element  mass  is  calculated  by 
abs(MASS) × ρ. 
NID 
PID 
MASS 
Remarks: 
1.  Axisymmetric  SPH,  IDIM = -2  in  CONTROL_SPH,  is  defined  on  global  X-Y 
plane, with Y-axis as the axis of rotation.  An axisymmetric SPH element has a 
mass of Aρ, where ρ is its density, A is the area of the SPH element and can be 
approximated by the area of its corresponding axisymmetric shell element, Fig.  
1.  The mass printout in d3hsp is the mass per radian, i.e., Aρxi, Fig.  1 & 2.
Y 
xi 
 A,ρ 
X 
1 rad 
xi 
Aρ 
X 
Axisymmetric SPH / corresponding shell 
Mass printout in d3hsp, mass/radian 
Mass printout in d3hsp, mass/radian
*ELEMENT_TRIM 
NOTE:  This keyword was replaced by *CONTROL_FORM-
ING_TRIMING starting in Revision 87566.
*ELEMENT_TSHELL_{OPTION} 
Available options include: 
<BLANK>  
BETA 
COMPOSITE 
Purpose:  Define an eight node thick shell element which is available with either fully 
reduced or selectively reduced integration rules.  Thick shell formulations 1, 2, and 6 are 
plane stress elements that can be used as an alternative to the 4 node shell elements in 
cases  where  an  8-node  element  is  desired.    Thick  shell  formulations  3,  5  and  7  are 
layered  solids  with  3D  stress  updates.    Formulation  5,  6,  and  7  are  based  on  an 
enhanced strain.  The number of through-thickness integration points is specified by the 
user. 
For orthotropic and anisotropic materials, a local material angle (variable BETA) can be 
defined which is cumulative with the integration point angles specified in *SECTION_-
TSHELL or *PART_COMPOSITE_TSHELL.   
The  COMPOSITE  option  for  *ELEMENT_TSHELL  allows  a  unique  stackup  of 
integration points for each element sharing the same part ID, and is available only when 
combined with *PART.   The COMPOSITE option is not available in combination with 
*PART_COMPOSITE_TSHELL.  To  maintain  a  direct  association  of  through-thickness 
integration  point  numbers  with  physical  plies  in  the  case  where  the  number  of  plies 
varies from element to element, see Remark 5. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
9 
Variable 
EID 
PID 
N1 
N2 
N3 
N4 
N5 
N6 
N7 
10 
N8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none  none  none  none  none  none  none  none  none  none 
Remarks
Beta Card.  Additional card for BETA keyword option. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
Type 
Default 
Remarks 
BETA 
F 
0. 
4 
Composite Card.  Additional card for COMPOSITE keyword option.  The material ID, 
thickness,  and  material  angle  for  each  through-thickness  integration  point  of  a 
composite  shell  are  defined.    The  integration  point  data  should  be  given  sequentially 
starting with the bottommost integration point.  The total number of integration points 
is  determined  by  the  number  of  entries  on  these  cards.      The  total  thickness  is  the 
distance  between  the  top  and  bottom  surface  as  determined  by  the  element 
connectivity, so the THICKi values are scaled to fit the element.  Define as many cards 
as needed.  The input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
Variable 
MID1 
THICK1 
Type 
I 
  Card 2 
1 
F 
2 
Variable 
MID3 
THICK3 
Type 
I 
F 
3 
B1 
F 
3 
B3 
F 
4 
5 
6 
MID2 
THICK2 
F 
6 
I 
5 
Etc. 
4 
7 
B2 
F 
7 
I 
F 
F 
8 
8 
  VARIABLE   
DESCRIPTION
EID 
PID 
N1 
Element ID.  Unique numbers have to be used. 
Part ID, see *PART. 
Nodal point 1
n5
n1
n8
n4
n6
n2
n7
n3
Figure 17-31.  8-node Thick Shell Element. 
  VARIABLE   
DESCRIPTION
N2 
N3 
⋮ 
N8 
BETA 
Nodal point 2 
Nodal point 3 
⋮  
Nodal point 8 
Orthotropic material base offset angle .  The angle 
is given in degrees.  If blank the default is set to zero. 
MIDi 
Material ID of integration point i, see the *MAT_… cards. 
THICKi 
Thickness of integration point i 
Bi 
Material angle of integration point i 
Remarks: 
1.  Orientation.  Extreme care must be used in defining the connectivity to ensure 
proper orientation of the through-thickness direction.  For a hexahedron, nodes 
𝑛1 to 𝑛4 define the lower surface, and nodes 𝑛5 to 𝑛8 define the upper surface.  
For  a  pentahedron,  nodes  𝑛1,  𝑛2,  𝑛3  form  the  lower  triangular  surface  and  the 
eight variables N1 to N8  should be defined using nodes 𝑛1, 𝑛2, 𝑛3, 𝑛3, 𝑛4, 𝑛5, 𝑛6, 
𝑛6, respectively.  Note that node 𝑛3 and node 𝑛6 are each repeated. 
2. 
Integration.  Element formulations 1 and 5 , use one 
point integration and the integration points then lie along the 𝑡-axis as shown in
Figure 17-31.  Element forumulations 2 and 3 use two by two selective reduced 
integration in each layer. 
3.  Stress  Output.    The  stresses  for  thick  shell  elements  are  output  in  the  global 
coordinate system.  
4.  Local  Coordinate  System.    To  allow  the  orientation  of  orthotropic  and 
anisotropic materials to be defined for each thick shell element, a beta angle can 
be  defined.    This  beta  angle  is  used  with  the  AOPT  parameter  and  associated 
data  on  the  *MAT  card  to  determine  an  element  reference  direction  for  the 
element. 
The AOPT data defines a coordinate system and the BETA angle defines a sub-
sequent rotation about the element normal to determine the element reference 
system.  For composite modeling, each layer in the element can have a unique 
material  direction  by defining  an  additional  rotation  angle  for the  layer,  using 
either the ICOMP and Bi parameters on *SECTION_TSHELL or the Bi parame-
ter on *PART_COMPOSITE_TSHELL.  The material direction for layer i is then 
determined by a rotation angle, 𝜃𝑖. 
5.  Assignment  of  Zero  Thickness  to  Integration  Points.    The  ability  to  assign 
zero- thickness integration points in the stacking sequence allows the number of 
integration points to remain constant even as the number of physical plies var-
ies  from  element  to  element  and  eases  post-processing  since  a  particular  inte-
gration  point  corresponds  to  a  physical  ply.    Such  a  capability  is  important 
when  one  or  more  of  the  physical  plies  are  not  continuous  across  a  part.    To 
represent  a  missing  ply  in  *ELEMENT_TSHELL_COMPOSITE,  set  THICKi  to 
0.0 for the corresponding integration point and additionally, set MID to -1.  
When  postprocessing  the  results  using  LS-PrePost  version  4.5,  read  both  the 
keyword deck and d3plot database into the code and then select    Option > N/A 
gray  fringe.    Then,  when  viewing  fringe  plots  for  a  particular  integration  point 
(FriComp > IPt > intpt#),  the  element  will  be  grayed  out  if  the  selected  integra-
tion point is missing (or has zero thickness) in that element.
*END 
The  *END  command  is  optional  and  signals  the  conclusion  of  a  keyword  input  file.  
Data in a keyword file beyond a *END command are not read by LS-DYNA.
Please see LS-DYNA Keyword User’s Manual, Volume II (Material Models).
Purpose:    The  keyword  *FREQUENCY_DOMAIN  provides  a  way  of  defining  and 
solving frequency domain vibration and acoustic problems.  The keyword cards in this 
section are defined in alphabetical order: 
*FREQUENCY_DOMAIN_ACCELERATION_UNIT 
*FREQUENCY_DOMAIN_ACOUSTIC_BEM_{OPTION} 
*FREQUENCY_DOMAIN_ACOUSTIC_FEM 
*FREQUENCY_DOMAIN_ACOUSTIC_FRINGE_PLOT_{OPTION} 
*FREQUENCY_DOMAIN_ACOUSTIC_INCIDENT_WAVE 
*FREQUENCY_DOMAIN_ACOUSTIC_SOUND_SPEED 
*FREQUENCY_DOMAIN_FRF 
*FREQUENCY_DOMAIN_MODE_{OPTION} 
*FREQUENCY_DOMAIN_PATH 
*FREQUENCY_DOMAIN_RANDOM_VIBRATION_{OPTION} 
*FREQUENCY_DOMAIN_RESPONSE_SPECTRUM 
*FREQUENCY_DOMAIN_SSD
*FREQUENCY_DOMAIN_ACCELERATION_UNIT 
Purpose:  LS-DYNA’s default behavior is to assume that accelerations are derived: 
[acceleration unit] =
[length unit]
[time unit]2 . 
This card extends LS-DYNA to support other units for acceleration. 
  Card 1 
1 
2 
Variable 
UNIT 
UMLT 
Type 
I 
F 
  VARIABLE   
DESCRIPTION
UNIT 
Flag for acceleration unit conversion: 
EQ.0:  use [length unit]/[time unit]2 as unit of acceleration. 
EQ.1:  use 𝑔 as unit for acceleration, and SI units (Newton, kg,
meter, second, etc.) elsewhere. 
EQ.2:  use 𝑔 as unit for acceleration, and Engineering units (lbf,
lbf × second2/inch, inch, second, etc.) elsewhere. 
EQ.3:  use  𝑔  as  unit  for  acceleration,  and  units  (kN,  kg,  mm,
ms, GPa, etc.) elsewhere. 
EQ.-1:  use 𝑔 as unit for acceleration and provide the multiplier
for converting g to [length unit]/[time unit]2. 
UMLT 
Multiplier  for  converting  𝑔  to  [length  unit]/[time  unit]2  (used 
only for UNIT = -1). 
Remarks: 
LS-DYNA uses consistent units.  With consistent units acceleration is defined using: 
[acceleration unit] =
[length unit]
[time unit]2 . 
However, it is the convention of many industries to use 𝑔 (gravitational acceleration on 
the Earth’s surface) as the base unit for acceleration.  Usually, data from vibration tests, 
both  random  and  sine  sweep,  are  expressed  in  systems  for  which  𝑔  is  the  unit  of 
acceleration.  With this keyword, LS-DYNA supports such conventions.  Internally, LS-
DYNA implements this keyword by converting the input deck into consistent units, and
then proceeding with the calculation as usual.  However, results are output in the unit 
system specified with this keyword.
*FREQUENCY_DOMAIN_ACOUSTIC_BEM_{OPTION1}_{OPTION2} 
Available options include: 
ATV 
MATV 
HALF_SPACE 
PANEL_CONTRIBUTION 
Purpose:    Activate  the  boundary  element  method  in  frequency  domain  for  acoustic 
problems.  This keyword is ignored unless the BEM=filename option is included in the 
LS-DYNA command line: 
Control Card.  To use this card LS-DYNA must be run with a BEM option, as in “LS-
DYNA I=inf  BEM=filename”. 
3 
4 
5 
6 
7 
8 
FMIN 
FMAX 
NFREQ 
DTOUT 
TSTART 
PREF 
  Card 1 
Variable 
1 
RO 
Type 
F 
2 
C 
F 
F 
F 
I 
0 
F 
0 
Default 
none 
none 
none 
none 
Remark 
F 
0 
1 
7 
F 
0 
2 
8 
  Card 2 
1 
2 
3 
4 
5 
6 
Variable  NSIDEXT 
TYPEXT 
NSIDINT 
TYPINT 
FFTWIN 
TRSLT 
IPFILE 
IUNITS 
I 
0 
I 
0 
I 
0 
I 
0 
Type 
Default 
Remark 
I 
0 
I 
0 
3 
I 
0 
4 
I 
0
Additional card for FFTWIN = 5. 
  Card 2a 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
T_HOLD 
DECAY 
Type 
F 
F 
Default 
0.0 
0.02 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  METHOD  MAXIT 
TOLITR 
NDD 
TOLLR 
TOLFCT 
IBDIM 
NPG 
Type 
I 
I 
F 
Default 
100 
10-4 
Remark 
6 
  Card 4 
1 
2 
3 
I 
1 
7 
4 
F 
F 
I 
10-6 
10-6 
1000 
I 
2 
5 
6 
7 
8 
Variable 
NBC 
RESTRT 
IEDGE 
NOEL 
NFRUP 
VELOUT 
DBA 
Type 
Default 
Remark 
I 
1 
I 
0 
8 
I 
0 
9 
I 
0 
I 
0 
I 
0 
I 
0 
10 
11
Boundary Condition Cards.  The deck must include NBC cards in this format: one for 
each boundary condition. 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
SSTYPE 
NORM 
BEMTYP 
LC1 
LC2 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
I 
Remark 
12 
Panel Contribution Card.  Additional for PANEL_CONTRIBUTION keyword option. 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSIDPC 
Type 
Default 
I 
0 
Remark 
13 
Half Space Card.  Additional card for HALF_SPACE keyword option. 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
Type 
Default 
I 
0 
  VARIABLE   
DESCRIPTION
RO 
Fluid density.
VARIABLE   
DESCRIPTION
C 
Sound speed of the fluid. 
GT.0: real constant sound speed. 
LT.0:  |C|  is  the  load  curve  ID,  which  defines  the  frequency
dependent  complex  sound  speed.    See  *FREQUENCY_-
DOMAIN_ACOUSTIC_SOUND_SPEED. 
FMIN 
FMAX 
Minimum value of output frequencies. 
Maximum value of output frequencies. 
NFREQ 
Number of output frequencies. 
DTOUT 
TSTART 
PREF 
Time  interval  between  writing  velocity  or  acceleration,  and
pressure at boundary elements in the binary file, to be proceeded
at the end of LS-DYNA simulation. 
Start  time  for  recording  velocity  or  acceleration  in  LS-DYNA 
simulation. 
Reference pressure to be used to output pressure in dB, in the file
Press_dB.  If PREF = 0, the Press_dB file will not be generated.  A 
file called Press_Pa is generated and contains the pressure at the 
output nodes . 
NSIDEXT 
Node or segment set ID of output exterior field points. 
TYPEXT 
Output exterior field point type. 
EQ.0: node ID. 
EQ.1: node set ID. 
EQ.2: segment set ID. 
NSIDINT 
Node or segment set ID of output interior field points. 
TYPINT 
Output interior field point type. 
EQ.0: node ID. 
EQ.1: node set ID. 
EQ.2: segment set ID.
VARIABLE   
DESCRIPTION
FFTWIN 
FFT windows (Default = 0). 
EQ.0: rectangular window. 
EQ.1: Hanning window. 
EQ.2: Hamming window. 
EQ.3: Blackman window. 
EQ.4: raised cosine window. 
EQ.5: exponential window. 
TRSLT 
Request time domain results: 
EQ.0: no time domain results are requested. 
EQ.1: time  domain  results  are  requested  (Press_Pa_t  gives 
absolute value pressure vs.  time). 
EQ.2: time domain results are requested (Press_Pa_t gives real 
value pressure vs.  time).
VARIABLE   
DESCRIPTION
IPFILE 
Flag for output files (default = 0): 
EQ.0:  Press_Pa  (magnitude  of  pressure  vs. 
  frequency), 
Press_dB  (sound  pressure  level  vs.    frequency)  and 
bepres (ASCII database file for LS-Prepost) are provid-
ed. 
EQ.1:  Press_Pa_real  (the  real  part  of  the  pressure  vs. 
frequency)  and  Press_Pa_imag  (the  imaginary  part  of 
the pressure vs.  frequency) are provided, in addition to
Press_Pa, Press_dB and bepres. 
EQ.10:  files  for  IPFILE = 0,  and  fringe  files  for  acoustic 
pressure. 
EQ.11:  files  for  IPFILE = 1,  and  fringe  files  for  acoustic 
pressure. 
EQ.20:  files  for  IPFILE = 0,  and  fringe  files  for  sound  pressure 
level. 
EQ.21:  files  for  IPFILE = 1,  and  fringe  files  for  sound  pressure 
level. 
EQ.31:  files for IPFILE = 1, and fringe files for acoustic pressure 
(real part). 
EQ.41:  files for IPFILE = 1, and fringe files for acoustic pressure 
(imaginary part). 
IUNITS 
Flag for unit changes 
EQ.0: do not apply unit change. 
EQ.1: MKS units are used, no change needed. 
EQ.2: units: lbf × s2/in, inch, s, lbf, psi, etc.  are used, changed 
to MKS in BEM Acoustic computation. 
EQ.3: units:  kg,  mm,  ms,  kN,  GPa,  etc.    are  used,  changed  to
MKS in BEM acoustic computation. 
EQ.4: units: ton, mm, s, N, MPa, etc.  are used, changed to MKS
in BEM acoustic computation. 
T_HOLD 
Hold-off  period  before  the  exponential  window.    The  length  of
the  hold-off  period  should  coincide  with  the  pre-trigger  time  to 
reduce the effects of noise in the captured time domain data.  It is
only used when FFTWIN = 5.
VARIABLE   
DECAY 
DESCRIPTION
Decay  ratio  at  the  end  of  capture  duration.    For  example,  if  the
DECAY = 0.02, it means that the vibration is forced to decay to 2%
of  its  amplitude  within  the  capture  duration.    This  field  is  only
used when FFTWIN = 5. 
METHOD 
Method used in acoustic analysis 
EQ.0: Rayleigh method (very fast). 
EQ.1: Kirchhoff method coupled to FEM for acoustics (*MAT_-
ACOUSTIC).  See Remark 6. 
EQ.2: variational Indirect BEM. 
EQ.3: collocation BEM. 
EQ.4: collocation  BEM  with  Burton-Miller  formulation  for 
exterior problems (no irregular frequency phenomenon).
MAXIT 
Maximum number of iterations for iterative solver (default = 100) 
if METHOD ≥ 2. 
TOLITR 
Tolerance for the iterative solver.  The default value is 10−4. 
NDD 
Number of domain decomposition, used for memory saving.  For 
large  problems,  the  boundary  mesh  is  decomposed  into  NDD
domains  for  less  memory  allocation.    This  option  is  only  used  if
METHOD ≥ 2. 
TOLLR 
Tolerance 
for 
(default = 10−6). 
low  rank  approximation  of  dense  matrix
TOLFCT 
Tolerance in factorization of the low rank matrix (default = 10−6).
IBDIM 
Inner iteration limit in GMRES iterative solver (default = 1000). 
NPG 
NBC 
RESTRT 
Number of Gauss integration points (default = 2). 
Number of boundary condition cards.  See Card 5.  (default = 1). 
This  flag  is  used  to  save  an  LS-DYNA  analysis  if  the  binary 
output  file  in  the  (bem=filename)  option  has  not  been  changed 
(default = 0). 
EQ.0: LS-DYNA  time  domain  analysis 
generates a new binary file. 
is  processed  and
EQ.1: LS-DYNA  time  domain  analysis  is  not  processed.    The
VARIABLE   
DESCRIPTION
binary files from previous run are used.  The files include
the  binary  output  file  filename,  and  the  binary  file 
bin_velfreq, which saves the boundary velocity from FFT.
EQ.2: LS-DYNA  restarts  from  d3dump  file  by  using  “R=” 
command  line  parameter.    This  is  useful  when  the  last
run was interrupted by sense switches such as “sw1”. 
EQ.3: LS-DYNA reads in user provided velocity history saved
in an ASCII file, bevel. 
EQ.4: run  acoustic  computation  on  a  boundary  element  mesh
with velocity information given with a denser finite ele-
ment  mesh  in  last  run.    This  option  requires  both
“bem = filename”  and  “lbem = filename2”  in  the  com-
mand line, where filename2 is the name of the binary file 
generated in the last run with denser mesh. 
EQ.5: LS-DYNA  time  domain  analysis  is  not  processed.    The
binary file filename from previous run is used.  An FFT is 
performed  to  get  the  new  frequency  domain  boundary
velocity and the results are saved in bin_velfreq. 
IEDGE 
Free edge and multi-connection constraints option (default = 0). 
EQ.0: free 
edge  and  multi-connection 
constraints  not 
considered. 
EQ.1: free edge and multi-connection constraints considered. 
EQ.2: only free edge constraints are considered. 
EQ.3: only multi-connection constraints are considered. 
NOEL 
Location  where  normal  velocity  or  acceleration 
(default = 0). 
is 
taken
EQ.0: elements or segments. 
EQ.1: nodes. 
NFRUP 
Preconditioner update option. 
EQ.0:  updated at every frequency. 
GE.1:  updated for every NFRUP frequencies.
VARIABLE   
DESCRIPTION
VELOUT 
Flag for writing out nodal or elemental velocity data. 
EQ.0: No writing out velocity data. 
EQ.1: write  out  time  domain  velocity  data  (in  𝑥,  𝑦  and  𝑧
directions). 
EQ.2: write  out  frequency  domain  velocity  data  (in  normal 
direction). 
DBA 
Flag  for  writing  out  weighted  SPL  files  with  different  weighting
options. 
EQ.0: No writing out weighted SPL files. 
EQ.1: write out Press_dB(A) by using A-weighting. 
EQ.2: write out Press_dB(B) by using B-weighting. 
EQ.3: write out Press_dB(C) by using C-weighting. 
EQ.4: write out Press_dB(D) by using D-weighting. 
SSID 
Part, part set ID, or segment set ID of boundary elements. 
SSTYPE 
Boundary element type: 
EQ.0: part Set ID 
EQ.1: part ID 
EQ.2: segment set ID. 
NORM 
NORM  should  be  set  such  that  the  normal  vectors  point  away
from the fluid. 
EQ.0: normal vectors are not inverted (default). 
EQ.1: normal vectors are inverted.
VARIABLE   
DESCRIPTION
BEMTYP 
Type of input boundary values in BEM analysis. 
EQ.0: boundary velocity will be processed in BEM analysis. 
EQ.1: boundary acceleration will be processed in BEM analysis.
EQ.2: pressure  is  prescribed  and  the  real  and  imaginary  parts
are given by LC1 and LC2. 
EQ.3: normal velocity is prescribed and the real and imaginary
parts are given by LC1 and LC2. 
EQ.4: impedance  is  prescribed  and  the  real  and  imaginary
parts are given by LC1 and LC2. 
LT.0:  normal  velocity  (only  real  part)  is  prescribed,  through
load  curve  n.    An  amplitude  as  a  function  of  frequency
load curve with curve ID |BEMTYP|. 
Load curve ID for defining real part of pressure, normal velocity
or impedance. 
Load  curve  ID  for  defining  imaginary  part  of  pressure,  normal
velocity or impedance. 
Node set ID for the field points where panel contributions to SPL
(Sound Pressure Level) are requested. 
Plane  ID  for  defining  the  half-space  problem,  see  keyword  *DE-
FINE_PLANE. 
LC1 
LC2 
NSIDPC 
PID 
Remarks: 
1.  TSART Field.  TSTART indicates the time at which velocity or acceleration and 
pressure are stored in the binary file. 
2.  PREF  Field.    This  reference  pressure  is  required  for  the  computation  of  the 
pressure in dB.  Usually, in International Unit System the reference pressure is 
20𝜇Pa. 
3.  FFT Windowing.  Velocity or acceleration (pressure) is provided by LS-DYNA 
analysis.    They  are  written  in  a  binary  file  (bem=filename).    The  boundary 
element method is processed after the LS-DYNA analysis.  An FFT algorithm is 
used to transform time domain data into frequency domain in order to use the 
boundary element method for acoustics.  In order to overcome the FFT leakage 
problem  due  to  the  truncation  of  the  temporal  response,  several  windows  are
Figure 20-1.  T-section. 
proposed.    Windowing  is  used  to  have  a  periodic  velocity,  acceleration  and 
pressure in order to use the FFT. 
4.  TRSLT Field.  If time domain results are requested, FMIN is changed to 0 in the 
code. 
5. 
IUNITS  Field.    Units  are  automatically  converted  into  kg,  m,  s,  N,  and  Pa  so 
that the reference pressure will not be too small.  For example, it may be as low 
as  20.E-15  GPa  if  one  uses  the  units  kg,  mm,  ms,  kN,  and  GPa  and  this  may 
result  in  truncation  error  in  the  computation,  especially  in  single  precision 
version. 
6.  METHOD  Field.    The  Rayleigh  method  is  an  approximation  suitable  only  for 
external  radiation  problems.    It  is  very  fast  since  there  is  no  linear  system  to 
solve.  The Kirchhoff method involves coupling the BEM and FEM for acoustics 
(*MAT_ACOUSTIC) with a Non Reflecting Boundary condition, see *BOUND-
ARY_NON_REFLECTING.    In  this  case,  at  least  one  fluid  layer  with  non-
reflecting  boundary  condition  is  merged  with  the  vibrating  structure.    This 
additional fluid is given in *MAT_ACOUSTIC by the same density and sound 
speed  as  used  in  this  keyword.    When  used  appropriately  both  methods  pro-
vide a good approximation to a full BEM calculation for external problems.  
7.  NDD Field.  BEM formulation for large and medium size problems (more than 
2000  boundary  elements)  is  memory  and  time  consuming.    In  this  case,  user 
may  run  LS-DYNA  using  the  memory  option.    In  order  to  save  memory,  do-
main decomposition can be used. 
8.  RESTRT Field.  The binary file generated by a previous run can be used for the 
next run by using the restart option.  The restart option allows the user to use 
the  binary  file  generated  from  a  previous  calculation  in  order to run  BEM.    In 
this case, the frequency range can be changed.  However, the time paraemeters 
should not be modified between calculations. 
9. 
IEDGE  Field.    This  option  only  applies  to  METHOD = 2,  the  Variational 
Indirect BEM. 
10.  NOEL  Field.    This  field  specified  whether  the  element  or  nodal  velocity  (or 
acceleration)  is  taken  from  FEM  computation.    NOEL  should  be  0  if  Kirchhoff 
method  (METHOD = 1)  is  used  since  elemental  pressure  is  processed  in  FEM.
NOEL should be 0 if Burton-Miller collocation method (METHOD = 4) is used 
since  a  constant  strength  element  formulation  is  adopted.    In  other  cases,  it  is 
strongly recommended to use element velocity or acceleration (NOEL = 0) if “T-
Section” appears in boundary element mesh.  See Figure 20-1. 
11.  NFRUP  Field.    The  preconditioner  is  obtained  with  the  factorization  of  the 
influence coefficient matrix.  To conserve CPU time, It can be retained for sev-
eral  frequencies.    By  default  (NFRUP=0),  the  preconditioner  is  updated  for 
every  frequency.    Note  that  in  MPP  version,  the  preconditioner  is  updated 
every NFRUP frequencies on each processor. 
12.  Boundary  Condition  Cards.    The  Card  5  can  be  defined  if  the  boundary 
elements  are  composed  of  several  panels.    It  can  be  defined  multiple  times  if 
more than 2 panels are used.  Each card 5 defines one panel. 
13.  NSIDPC  Field.    The  field  points  where  the  panel  contribution  analysis  is 
requested must be one of the field points for acoustic computation (it must be 
included in the nodes specified by the NSIDEXT or NSIDINT).  The panels are 
defined by card 4 and card 5, etc.  Each card defines one panel. 
14.  Element  Sizing.    To  obtain  accurate  results,  the  element  size  should  not  be 
greater than 1/6 of the wave length  (= 𝑐/𝑓  where 𝑐 is the wave speed and 𝑓  
is the frequency). 
15.  Acoustic  Transfer  Vector.    The  Acoustic  Transfer  Vector  can  be  obtained  by 
including the option ATV in the keyword.  It calculates acoustic pressure (and 
sound pressure level) at field points due to unit normal velocity of each surface 
node.    ATV  is  dependent  on  structure  model,  properties  of  acoustic  fluid  as 
well  as  location  of  field  points.    When  ATV  option  is  included,  the  structure 
does  not  need  any  external  excitation,  and  the  curve  IDs  LC1  and  LC2  are  ig-
nored.  A binary plot database d3atv can be obtained by setting BINARY = 1 in 
*DATABASE_FREQUENCY_BINARY_D3ATV. 
16.  Modal  Acoustic  Transfer  Vector.    The  Modal  Acoustic  Transfer  Vector 
(MATV) is calculated when the MATV keyword option is included.  The MATV 
option  requires  that  the  implicit  eigenvalue  solver  be  used,  which  is  activated 
by  keywords  *CONTROL_IMPLICIT_GENERAL,  and  *CONTROL_IMPLIC-
IT_EIGENVALUE.  It calculates acoustic pressure (and sound pressure level) at 
field  points  due  to  vibration  in  the  form  of  eigenmodes.    For  each  excitation 
frequency  𝑓 ,  LS-DYNA  generates  the  psedo-velocity  boundary  condition 
2𝜋𝑖𝑓 {𝜙}𝑗,  where  𝑖 = √−1  is  the  imaginary  unit  and  runs  acoustic  computation 
for each field point, based on the psedo-velocity boundary conditions, to get the 
MATV matrices.  The MATV matrices are saved in binary file “bin_bepressure” 
for  future  use.    Like  ATV,  MATV  is  also  only  dependent  on  structure  model, 
properties of acoustic fluids as well as the location of field points.
17.  Output Files.  The result files: Press_Pa, Press_dB, Press_Pa_real, Press_Pa_
imag,  Press_Pa_t  and  Press_dB_t  have  a  xyplot  format  that  LS-PrePost  can 
read and plot.
*FREQUENCY_DOMAIN_ACOUSTIC_FEM_{OPTION} 
Available options include: 
EIGENVALUE 
Purpose:  Define an interior acoustic problem and solve the problem with a frequency 
domain  finite  element  method.    When  EIGENVALUE  option  is  used,  compute 
eigenvalues and eigenvectors of the acoustic system. 
  Card 1 
Variable 
1 
RO 
Type 
F 
2 
C 
F 
F 
F 
3 
4 
5 
6 
7 
8 
FMIN 
FMAX 
NFREQ 
DTOUT 
TSTART 
PREF 
Default 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
Variable 
FFTWIN 
I 
0 
5 
F 
0 
6 
F 
0 
7 
F 
0 
8 
Type 
Default 
  Card 3 
1 
I 
0 
2 
Variable 
PID 
PTYP 
Type 
I 
Default 
none 
I 
0 
3 
4 
5 
6 
7
Boundary  Condition  Definition  Card.    It  can  be  repeated  if  multiple  boundary 
conditions are present.  This card is optional when option EIGENVALUE is present. 
  Card 4 
1 
2 
3 
4 
5 
6 
Variable 
SID 
STYP 
VAD 
DOF 
LCID1 
LCID2 
Type 
I 
Default 
none 
I 
0 
I 
0 
I 
none 
I 
0 
I 
0 
7 
SF 
F 
1.0 
8 
VID 
I 
0 
Field Points Definition Card.  Not used when option EIGENVALUE is present. 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID 
NTYP 
IPFILE 
DBA 
Type 
I 
Default 
none 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
RO 
C 
Fluid density. 
Sound speed of the fluid. 
GT.0: real constant sound speed. 
LT.0:  |C|  is  the  load  curve  ID,  which  defines  the  frequency
dependent  complex  sound  speed.    See  *FREQUENCY_-
DOMAIN_ACOUSTIC_SOUND_SPEED. 
FMIN 
FMAX 
Minimum value of output frequencies. 
Maximum value of output frequencies. 
NFREQ 
Number of output frequencies. 
DTOUT 
Time step for writing velocity or acceleration in the binary file. 
TSTART 
Start  time  for  recording  velocity  or  acceleration  in  transient
analysis.
VARIABLE   
DESCRIPTION
PREF 
Reference pressure, for converting the acoustic pressure to dB. 
FFTWIN 
FFT windows (Default = 0): 
EQ.0: rectangular window. 
EQ.1: Hanning window. 
EQ.2:  Hamming window. 
EQ.3: Blackman window. 
EQ.4: Raised cosine window. 
PID 
PTYP 
Part ID, or part set ID to define the acoustic domain. 
Set type: 
EQ.0: part, see *PART. 
EQ.1: part set, see *SET_PART. 
SID 
Part ID, or part set ID, or segment set ID, or node set ID to define
the boundary where vibration boundary condition is provided 
STYP 
Set type: 
EQ.0: part, see *PART. 
EQ.1: part set, see *SET_PART. 
EQ.2: segment set, see *SET_SEGMENT. 
EQ.3: node set, see *SET_NODE. 
VAD 
Boundary condition flag: 
EQ.0:  velocity by steady state dynamics (SSD). 
EQ.1:  velocity by transient analysis. 
EQ.2:  opening (zero pressure). 
EQ.11:  velocity by LCID1 (amplitude) and LCID2 (phase). 
EQ.12:  velocity by LCID1 (real) and LCID2 (imaginary). 
EQ.21:  acceleration by LCID1 (amplitude) and LCID2 (phase). 
EQ.22:  acceleration by LCID1 (real) and LCID2 (imaginary). 
EQ.31:  displacement by LCID1 (amplitude) and LCID2 (phase).
EQ.32:  displacement by LCID1 (real) and LCID2 (imaginary).
VARIABLE   
DESCRIPTION
EQ.41:  impedance by LCID1 (amplitude) and LCID2 (phase). 
EQ.42:  impedance by LCID1 (real) and LCID2 (imaginary). 
EQ.51:  pressure by LCID1 (amplitude) and LCID2 (phase). 
EQ.52:  pressure by LCID1 (real) and LCID2 (imaginary). 
DOF 
Applicable degrees-of-freedom: 
EQ.0: determined by steady state dynamics. 
EQ.1: 𝑥-translational degree-of-freedom, 
EQ.2: 𝑦-translational degree-of-freedom, 
EQ.3: 𝑧-translational degree-of-freedom, 
EQ.4: translational motion in direction given by VID, 
EQ.5: normal direction of the element or segment. 
LCID1 
LCID2 
SF 
VID 
NID 
Load curve ID to describe the amplitude (or real part) of velocity,
see *DEFINE_CURVE. 
Load  curve  ID  to  describe  the  phase  (or  imaginary  part)  of 
velocity, see *DEFINE_CURVE. 
Load curve scale factor. 
Vector ID for DOF values of 4. 
Node  ID,  or  node  set  ID,  or  segment  set  ID  for  acoustic  result
output. 
NTYP 
Set type: 
EQ.0: Node, see *NODE. 
EQ.1: Node set, see *SET_NODE. 
IPFILE 
Flag for output files (default = 0): 
EQ.0: Press_Pa (magnitude of pressure vs.  frequency), Press_
dB (sound pressure level vs.  frequency) are provided. 
EQ.1: Press_Pa_real  (real  part  of  pressure  vs.    frequency)  and 
Press_Pa_imag (imaginary part of pressure vs.  frequen-
cy) are provided, in addition to Press_Pa, Press_dB.
VARIABLE   
DBA 
DESCRIPTION
Flag  for  writing  out  weighted  SPL  files  with  different  weighting
options. 
EQ.0: No writing out weighted SPL files. 
EQ.1: write out Press_dB(A) by using A-weighting. 
EQ.2: write out Press_dB(B) by using B-weighting. 
EQ.3: write out Press_dB(C) by using C-weighting. 
EQ.4: write out Press_dB(D) by using D-weighting. 
Remarks: 
1.  This  command  solves  the  interior  acoustic  problems  which  is  governed  by 
Helmholtz  equation  ∇2𝑝 + 𝑘2𝑝 = 0  with  the  boundary  condition  ∂𝑝 ∂𝑛⁄ =
−𝑖𝜔𝜌𝑣𝑛, where, 𝑝 is the acoustic pressure; 𝑘 = 𝜔/𝑐 is the wave number; 𝜔 is the 
round  frequency;  𝑐 is  the  acoustic  wave  speed  (sound  speed);  𝑖 = √−1 is  the 
imaginary unit; 𝜌 is the mass density and 𝑣𝑛 is the normal velocity.  This com-
mand solves the acoustic problem in frequency domain. 
2. 
If mass density RO is not given, the mass density of PID (the part which defines 
the acoustic domain), will be used  
3.  PREF  is  the  reference  pressure  to  convert  the  acoustic  pressure  to  dB  𝐿𝑝 =
) Note that generally 𝑝ref = 20𝜇Pa for air. 
2⁄
10 log10(𝑝2 𝑝ref
4. 
If  the  boundary  velocity  is  obtained  from  steady  state  dynamics  (VAD = 0) 
using  the  keyword  *FREQUENCY_DOMAIN_SSD,  the  part  (PID)  which  de-
fines the acoustic domain has to use one of the following material models,  
a)  MAT_ELASTIC_FLUID 
b)  MAT_NULL (and EOS_IDEAL_GAS) 
Since only the above material models enable implicit eigenvalue analysis.  If the 
boundary  excitation  is  given  by  load  curves  LCID1  and  LCID2  (VAD > 0),  the 
part (PID) which defines the acoustic domain can use any material model which 
is  compatible  with  8-node  solid  elements,  as  only  the  mesh  of  the  PID  will  be 
utilized in the computation.  For example, MAT_ACOUSTIC and MAT_ELAS-
TIC_FLUID can be used. 
5. 
If  VAD = 0,  the  boundary  excitation  is  given  as  velocity  obtained  from  steady 
state dynamics.  The other parameters in Card 3 (DOF, LCID1, LCID2, SF and 
VID) are ignored.
6. 
If a node’s vibration boundary condition is defined multiple times, only the last 
definition  is  considered.    This  happens  usually  when  a  node  is  on  edge  and 
shared by two or more PART, SET_PART, SET_NODE, or SET_SEGMENT and 
different vibration condition is defined on each of the SET_NODE or SET_SEG-
MENT. 
SET_SEGMENT 1
NODE shared by two 
SET_SEGMENT 
SET_SEGMENT 2 
7.  Results  including  acoustic  pressure  and  SPL  are  given  in  d3acs  binary  files, 
which can be accessed by LS-PrePost.  Nodal pressure and SPL values for nodes 
specified  by  NID  and  NTYP  are  given  in  ASCII  file  Press_Pa  and  Press_dB, 
which  can  be  accessed  by  LS-PrePost.    Press_Pa  gives  magnitude of  the  pres-
sure.  Press_dB gives Sound Pressure Level in terms of dB. 
8. 
If  the  boundary  velocity  condition  is  given  by  Steady  State  Dynamics 
(VAD = 0),  the  range  and  number  of  frequencies  (FMIN,  FMAX  and  NFREQ) 
should be compatible with the corresponding parameters in Card 1 of the key-
word *FREQUENCY_DOMAIN_SSD 
9.  For acoustic eigenvalue analysis (OPTION = EIGENVALUE), Card 4 is optional 
and Card 5 is not used.
*FREQUENCY_DOMAIN_ACOUSTIC_FRINGE_PLOT_{OPTION} 
Available options include: 
PART 
PART_SET 
NODE_SET 
SPHERE 
PLATE 
Purpose:  Define field points for acoustic pressure computation by BEM acoustic solver, 
and save the results to D3ACS binary database. 
Card 1 for option PART, PART_SET or NODE_SET. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID/SID 
Type 
I 
Default 
none 
Card 1 for option SPHERE. 
  Card 1 
1 
Variable 
CENTER 
Type 
Default 
I 
1 
2 
R 
F 
3 
DENSITY 
I 
4 
X 
F 
5 
Y 
F 
6 
Z 
F 
7 
8 
none 
none 
none 
none 
none 
Card 1 for option PLATE.
Card 1 
1 
2 
3 
Variable 
NORM 
LEN_X 
LEN_Y 
Type 
Default 
I 
1 
F 
F 
4 
X 
F 
5 
Y 
F 
6 
Z 
F 
7 
8 
NELM_X  NELM_Y 
I 
I 
none 
none 
none 
none 
none 
10 
10 
  VARIABLE   
DESCRIPTION
PID/SID 
Part ID or part set ID or node set ID. 
CENTER 
Flag for defining the center point for the sphere. 
EQ.1: mass center of the original structure. 
EQ.2:  geometry center of the original structure. 
EQ.3:  defined by (x, y, z). 
R 
Radius of the sphere. 
DENSITY 
Parameter to define how coarse or dense the created sphere mesh
is.    It  is  a  number  between  3  and  39,  where  “3”  gives  you  24
elements while “39” gives you 8664 elements. 
X 
Y 
Z 
x-coordinate of the center. 
y-coordinate of the center. 
z-coordinate of the center. 
NORM 
Norm direction of the plate.  
EQ.1: x-direction 
EQ.2:  y-direction 
EQ.3:  z-direction 
LEN_X 
Length of longer side of the plate. 
LEN_Y 
Length of shorter side of the plate. 
NELM_X 
Number of elements on longer side of the plate. 
NELM_Y 
Number of elements on shorter side of the plate.
Remarks: 
1.  This  command  defines  field  points  where  the  acoustic  pressure  will  be 
computed  by  *FREQUENCY_DOMAIN_ACOUSTIC_BEM.    The  field  points 
can be defined as existing structure components if option PART, PART_SET or 
NODE_SET  is  used.    The  field  points  can  be  created  by  LS-DYNA  if  option 
SPHERE or PLATE is used. 
2.  The  acoustic  pressure  results  at  those  field  points  are  saved  in  D3ACS  binary 
database and are accessible by LS-PrePost.  With FCOMP tool in LS-PrePost, the 
fringe  plot  of  the  results  (real  part  acoustic  pressure,  imaginary  part  acoustic 
pressure,  magnitude  of  acoustic  pressure  and  Sound  Pressure  Level)  can  be 
generated. 
3.  The  field  points  defined  by  this  keyword  are  separate  from  the  field  points 
defined in Card 2 of *FREQUENCY_DOMAIN_ACOUSTIC_BEM.  The acoustic 
pressure  results  for  the  latter  are  only  saved  in  ASCII  database  Press_Pa  and 
Press_dB,  etc.    (in  a  tabular  format  that  can  be  plotted  in  LS-PrePost  by  using 
the XYPlot tool).
*FREQUENCY_DOMAIN_ACOUSTIC_INCIDENT_WAVE 
Purpose:  Define incident sound wave for acoustic scattering problems. 
Wave Definition Cards.  This card may be repeated to define multiple incident waves. 
Input stops when the next “*” Keyword is found. 
  Card 1 
1 
2 
Variable 
TYPE 
MAG 
Type 
Default 
I 
1 
F 
6 
7 
8 
3 
XC 
F 
4 
YC 
F 
5 
ZC 
F 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
TYPE 
Type of incident sound wave: 
EQ.1: plane wave. 
EQ.2: spherical wave. 
MAG 
Magnitude of the incident sound wave. 
GT.0: constant magnitude. 
LT.0:  |MAG|  is  a  curve  ID,  which  defines  the  frequency
dependent magnitude.  See *DEFINE_CURVE. 
XC, YC, ZC 
Direction cosines for the place wave (TYPE = 1), or coordinates of 
the point source for the spherical wave (TYPE = 2). 
Remarks: 
1.  For plane wave, the incident wave is defined as 
𝑝(𝑥, 𝑦, 𝑧) = 𝐴𝑒−𝑖𝑘(𝛼𝑥+𝛽𝑦+𝛾𝑧) 
where, 𝐴 is the magnitude of the incident wave and 𝛼, 𝛽 and 𝛾 are the direction 
cosines along the incident direction. 𝑖 = √−1 is the imaginary unit and 𝑘 = 𝜔/𝑐  
is the wave number. 𝜔 is the round frequency and 𝑐 is the sound speed. 
2.  For spherical wave, the incident wave is defined as 
𝑝(𝑟) = 𝐴
𝑒−𝑖𝑘𝑟
*FREQUENCY_DOMAIN_ACOUSTIC_INCIDENT_WAVE  *FREQUENCY_DOMAIN 
where, 𝐴 is the magnitude of the incident wave and 𝑟 is the distance measured 
from the position of the point source.
*FREQUENCY_DOMAIN_ACOUSTIC_SOUND_SPEED 
Purpose:    Define  frequency  dependent  complex  sound  speed  to  be  used  in  frequency 
domain finite element method or boundary element method acoustic analysis. 
2 
3 
4 
5 
6 
7 
8 
  Card 1 
Variable 
1 
ID 
Type 
I 
Default 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID1 
LCID2 
Type 
I 
I 
Default 
none 
none 
  VARIABLE   
DESCRIPTION
Complex sound speed ID. 
Curve  ID  for  real  part  of  frequency  dependent  complex  sound 
speed. 
Curve  ID  for  imaginary  part  of  frequency  dependent  complex
sound speed. 
ID 
LCID1 
LCID2 
Remarks: 
1.  The  sound  speed  in  an  acoustic  medium  is  usually  defined  as  a  constant  real 
value.    But  it  can  also  be  defined  as  a  complex  value  which  is  dependent  on 
frequency, to introduce damping in the system. 
2.  To  use  the  frequency  dependent  complex  sound  speed  defined  here,  set  the 
sound  speed  C = -ID  in  *FREQUENCY_DOMAIN_ACOUSTIC_FEM,  or  *FRE-
QUENCY_DOMAIN_ACOUSTIC_BEM keywords.
*FREQUENCY_DOMAIN_FRF 
Purpose:    This  keyword  computes  frequency  response  functions  due  to  nodal 
excitations. 
NOTE:  Natural frequencies and mode shapes are needed for 
computing  the  frequency  response  functions.    Thus, 
*CONTROL_IMPLICIT_EIGENVALUE 
keyword 
must be included in input.  See Remark 1. 
  Card 1 
Variable 
1 
N1 
Type 
I 
Default 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
N1TYP 
DOF1 
VAD1 
VID1 
FNMAX  MDMIN  MDMAX 
I 
0 
2 
I 
none 
3 
I 
3 
4 
I 
0 
5 
F 
0.0 
6 
I 
0 
7 
I 
0 
8 
Variable 
DAMPF 
LCDAM 
LCTYP 
DMPMAS DMPSTF 
Type 
F 
Default 
0.0 
  Card 3 
Variable 
1 
N2 
I 
0 
2 
I 
0 
3 
F 
F 
0.0 
0.0 
4 
5 
6 
7 
8 
N2TYP 
DOF2 
VAD2 
VID2 
RELATV 
Type 
I 
Default 
none 
I 
0 
I 
none 
I 
2 
I 
0 
I
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FMIN 
FMAX 
NFREQ 
FSPACE 
LCFREQ 
RESTRT 
OUTPUT 
Type 
F 
F 
Default 
none 
none 
I 
2 
I 
0 
I 
none 
I 
0 
I 
0 
  VARIABLE   
N1 
DESCRIPTION
Node  /  Node  set/Segment  set  ID  for  excitation  input.    When
VAD1,  the  excitation  type,  is  set  to  1,  which  is  acceleration,  this
field is ignored. 
N1TYP 
Type of N1: 
EQ.0: node ID, 
EQ.1: node set ID, 
EQ.2: segment set ID. 
When VAD1, the excitation type, is set to 1, which is acceleration,
this field is ignored. 
DOF1 
Applicable  degrees-of-freedom  for  excitation  input  (ignored  if 
VAD1 = 4): 
EQ.0: 
translational  movement  in  direction  given  by  vector
VID1, 
EQ.1:  x-translational  degree-of-freedom,  or  x-rotational 
degree-of-freedom (for torque excitation, VAD1 = 8) 
EQ.2:  y-translational  degree-of-freedom,  or  y-rotational 
degree-of-freedom (for torque excitation, VAD1 = 8), 
EQ.3:  z-translational  degree-of-freedom,  or 
z-rotational 
degree-of-freedom (for torque excitation, VAD1 = 8).
VARIABLE   
DESCRIPTION
VAD1 
Excitation input type: 
EQ.0: base velocity, 
EQ.1: base acceleration, 
EQ.2: base displacement, 
EQ.3: nodal force, 
EQ.4: pressure, 
EQ.5: enforced velocity by large mass method, 
EQ.6: enforced acceleration by large mass method, 
EQ.7: enforced displacement by large mass method. 
EQ.8:  torque, 
EQ.9: base angular velocity, 
EQ.10: 
EQ.11: 
base angular acceleration, 
base angular displacement 
VID1 
FNMAX 
MDMIN 
MDMAX 
Vector  ID  for  DOF1 = 0  for  excitation  input,  see  *DEFINE_VEC-
TOR. 
Optional  maximum  natural 
computation.  See Remark 3. 
frequency  employed 
in  FRF
The  first  mode  employed  in  FRF  computation  (optional).    See
Remarks 3 and 4. 
The  last  mode  employed  in  FRF  computation  (optional).    It
should be set as a positive integer in a restart run (RESTRT = 1 or 
3)  based  on  the  number  of  eigenmodes  available  in  the  existing
d3eigv database.  See Remarks 3 and 4. 
DAMPF 
Modal damping coefficient, 𝜁 .  See Remark 5. 
LCDAM 
Load  Curve  ID  defining  mode  dependent  modal  damping
coefficient, 𝜁 .  See Remark 5. 
LCTYP 
Type of load curve defining modal damping coefficient: 
EQ.0: Abscissa value defines frequency, 
EQ.1: Abscissa value defines mode number. 
See Remark 5.
VARIABLE   
DMPMAS 
DESCRIPTION
Mass  proportional  damping  constant,  𝛼,  in  Rayleigh  damping. 
See Remark 5. 
DMPSTF 
Stiffness proportional damping constant, 𝛽, in Rayleigh damping. 
See Remark 5. 
N2 
Node / Node set/Segment set ID for response output. 
N2TYP 
Type of N2: 
EQ.0: node ID, 
EQ.1: node set ID, 
EQ.2: segment set ID. 
DOF2 
Applicable degrees-of-freedom for response output: 
EQ.0: direction given by vector VID2, 
EQ.1: 𝑥-translational degree-of-freedom, 
EQ.2: 𝑦-translational degree-of-freedom, 
EQ.3: 𝑧-translational degree-of-freedom, 
EQ.4: 𝑥-rotational degree-of-freedom, 
EQ.5: 𝑦-rotational degree-of-freedom, 
EQ.6: 𝑧-rotational degree-of-freedom, 
EQ.7: 𝑥, 𝑦 and 𝑧-translational degrees-of-freedom, 
EQ.8: 𝑥, 𝑦 and 𝑧-rotational degrees-of-freedom. 
VAD2 
Response output type: 
EQ.0: velocity, 
EQ.1: acceleration, 
EQ.2: displacement,  
EQ.3: nodal force . 
VID2 
Vector  ID  for  DOF2 = 0  for  response  direction,  see  *DEFINE_-
VECTOR. 
RELATV 
FLAG for displacement, velocity and acceleration results: 
EQ.0: absolute values are requested, 
EQ.1: relative values are requested (for VAD1 = 0, 1, 2 only).
VARIABLE   
DESCRIPTION
FMIN 
FMAX 
Minimum frequency for FRF output (cycles/time).  See Remark 6.
Maximum frequency for FRF output (cycles/time).  See Remark 6.
NFREQ 
Number of frequencies for FRF output.  See Remark 6. 
FSPACE 
Frequency spacing option for FRF output: 
EQ.0: linear, 
EQ.1: logarithmic, 
EQ.2: biased. 
See Remark 6. 
LCFREQ 
Load  Curve  ID  defining  the  frequencies  for  FRF  output.    See
Remark 6. 
RESTRT 
Restart option: 
EQ.0: initial run, 
EQ.1: restart with d3eigv family files, 
EQ.2: restart with dumpfrf, 
EQ.3: restart with d3eigv family files and dumpfrf. 
See Remark 7. 
OUTPUT 
Output option: 
EQ.0: write amplitude and phase angle pairs, 
EQ.1: write real and imaginary pairs. 
Remarks: 
1.  Frequency Response Functions.  The FRF (frequency response functions) can 
be  given  as  Displacement/Force  (called  Admittance,  Compliance,  or  Re-
ceptance), Velocity/Force (called Mobility), Acceleration/Force (called Acceler-
ance, Inertance), etc. 
2.  Enforced  Motion.    The  excitation  input  can  be  given  as  enforced  motion 
(VAD1 = 5, 6, 7).  Large mass method is used for this type of excitation input.  
The user need to attach a large mass to the nodes where the enforced motion is 
applied  by  using  the  keyword  *ELEMENT_MASS_{OPTION},  and  report  the 
keyword 
large 
(MPN) 
node 
mass 
per 
the 
in
*CONTROL_FREQUENCY_DOMAIN. 
*CONTROL_FREQUENCY_DOMAIN. 
  For  more  details,  please  refer  to 
3.  Maximum  Frequency.    FNMAX  decides  how  many  natural  vibration  modes 
are  adopted  in  FRF  computation.    LS-DYNA  uses  only  modes  with  lower  or 
equal frequency than FNMAX in FRF computation.  If FNMAX is not given, the 
number of modes in FRF computation is same as the number of modes, NEIG, 
from the *CONTROL_IMPLICIT_EIGENVALUE keyword card, unless MDMIN 
and MDMAX are prescribed . 
4.  Maximum/Minimum Mode.  MDMIN and MDMAX decide which mode(s) are 
adopted in FRF computation.  This option is useful for calculating the contribu-
tion  from  a  single  mode  (MDMIN  =  MDMAX)  or  several  modes  (MDMIN  < 
MDMAX).  If only MDMIN is given, LS-DYNA uses the single mode (MDMIN) 
to compute FRF.  In a restart run based on existing eigenmode database d3eigv 
(RESTRT  =  1  or  3),  MDMAX  should  be  a  positive  integer  which  is  equal  to or 
less than the number of eigenmodes available in d3eigv. 
5.  Damping.  Damping can be prescribed in several ways:  
a)  To  use  a  constant  modal  damping  coefficient  ζ  for  all  the  modes,  define 
DAMPF only.  LCDMP, LCTYP, DMPMAS and DMPSTF are ignored. 
b)  To use mode dependent modal damping, define a load curve (*DEFINE_-
CURVE)  and  specify  that  if  the  abscissa  value  defines  the  frequency  or 
mode number by LCTYP.  DMPMAS and DMPSTF are ignored. 
c)  To  use  Rayleigh  damping,  define  DMPMAS  (𝛼)  and  DMPSTF  (𝛽)  and 
keep DAMPF as 0.0, and keep LCDMP, LCTYP as 0.  The damping matrix 
in Rayleigh damping is defined as 𝐂 = 𝛼𝐌 + 𝛽𝐊, where, 𝐂, 𝐌 and 𝐊 are 
the damping, mass and stiffness matrices respectively.
fmin
fmin
fmin
Linear Spacing
Logarithmic Spacing
fmax
fmax
mode n
mode n+1
mode n+2
Biased Spacing
fmax
Figure 20-2.  Spacing options of the frequency points. 
6.  Frequency Points.  There are two methods to define the frequencies. 
a)  The first method is to define FMIN, FMAX, NFREQ and FSPACE.  FMIN 
and  FMAX  specify  the  frequency  range  of  interest  and  NFREQ  specifies 
the  number  of  frequencies  at  which  results  are  required.    FSPACE  speci-
fies  the  type  of  frequency  spacing  (linear,  logarithmic  or  biased)  to  be 
used. 
These  frequency  points  for  which  results  are  required  can  be  spaced 
equally  along  the  frequency  axis  (on  a  linear  or  logarithmic  scale).    Or 
they can be biased toward the eigenfrequencies (the frequency points are 
placed closer together at eigenfrequencies in the frequency range) so that 
the detailed definition of the response close to resonance frequencies can 
be obtained.  See Figure 20-2. 
b)  The second method is to use a load curve (LCFREQ) to define the frequen-
cies of interest. 
7.  RESTRT Field.  To save time in subsequent runs, the modal analysis stored in 
the d3eigv file during the first run can be reused by setting RESTRT=1. 
RESTRT = 2 or 3 is used when user wants to add extra vibration modes to FRF 
computation.  After initial FRF computation, user may find that the number of 
vibration  modes  is  not  enough.    For  example,  in  the  initial  computation,  user 
may  use  only  vibration  modes  up  to  500  Hz.    Later  it  is  found  that  vibration 
modes at higher frequencies are needed.  Then it would be more efficient to just 
compute the extra modes (frequencies above 500 Hz), and add the contribution 
from these extra modes to the previous FRF results. 
In  this  case,  user  may  use  the  option  RESTRT = 2  or  3.    For  RESTRT = 2,  LS-
DYNA runs a new modal analysis, reads in the previous FRF results (stored in
the binary dump file dumpfrf), and add the contribution from the new modes.  
For  RESTRT = 3,  LS-DYNA  reads  in  d3eigv  family  files  generated  elsewhere 
and reads in also dumpfrf, and add the contribution from the new modes. 
8.  Nodal Force Response Output.  For nodal force response (VAD2=3), the same 
nodes  or  node  set  need  to  be  defined  in  *DATABASE_NODAL_FORCE_-
GROUP.  In addition the MSTRES field for the *CONTROL_IMPLICIT_EIGEN-
VALUE keyword must be set to 1.
*FREQUENCY_DOMAIN_MODE_{OPTION1}_{OPTION2} 
Available options for OPTION1 include: 
LIST 
GENERATE 
SET 
For OPTION2 the available option is: 
EXCLUDE 
Purpose: 
  Define  vibration  modes  to  be  used  in  modal  superposition,  modal 
acceleration  or  modal  combination  procedures  for  mode-based  frequency  domain 
analysis  (such  as  frequency  response  functions,  steady  state  dynamics,  random 
vibration  analysis  and  response  spectrum  analysis).    When  the  option2  EXCLUDE  is 
used, the modes defined in this keyword are excluded from participating in the modal 
superposition, modal acceleration or modal combination procedures. 
Mode ID Cards.  For LIST keyword option list the mode IDs.  Include as many cards as 
necessary.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID1 
MID2 
MID3 
MID4 
MID5 
MID6 
MID7 
MID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Mode  Block  Cards.    For  GENERATE  keyword  option  specify  ranges  of  modes. 
Include as many cards as necessary.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  M1BEG  M1END  M2BEG  M2END  M3BEG  M3END  M4BEG  M4END 
Type 
I 
I 
I 
I 
I 
I 
I
Mode Set Card.  For SET keyword option specify a mode set.  Include only one card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
Type 
I 
  VARIABLE   
DESCRIPTION
MIDn 
Mode ID n. 
MnBEG 
First mode ID in block n. 
MnEND 
Last  mode  ID  in  block  n.    All  mode  ID’s  between  and  including
MnBEG and MnEND are added to the list. 
SID 
Mode set identification . 
Remarks: 
1.  User may use this keyword if some of the vibration modes have less contribu-
tion to the total structural response and can be removed from the modal super-
position,  modal  acceleration  or  modal  combination  procedures  in  the  mode-
based frequency domain analysis. 
2.  The  mode  list  defined  by  this  keyword  overrides  the  modes  specified  by  MD-
MIN,  MDMAX  (or  FNMIX,  FNMAX)  in  the  keywords  *FREQUENCY_DO-
MAIN_FRF, *FREQUENCY_DOMAIN_SSD, etc.
*FREQUENCY_DOMAIN_PATH_{OPTION} 
Available options include: 
<BLANK> 
PARTITION 
Purpose:    Specify  the  path  and  file  name  of  binary  databases  (e.g.  d3eigv)  containing 
mode information for restarting frequency domain analyses such as FRF, SSD, Random 
vibration, and Response spectrum analysis. 
The  PARTITION  option  supports  assigning  different  binary  databases  to  different 
frequency  ranges.    Specifically,  each  frequency  range  can  be  associated  with  different 
eigenmodes  and  modal  shape  vectors  provided  by  the  binary  database.    This  option 
provides a model for materials that have frequency-dependent properties. 
Partition  Cards.    Card  1  for  the  PARTITION  keyword  option.    Include  one  card  for 
each frequency range.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FBEG 
FEND 
FILENAME 
Type 
F 
F 
Default 
none 
none 
C 
none 
Filename Card.  Card 1 format used with the keyword option left blank. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME 
C 
none 
  VARIABLE   
DESCRIPTION
FBEG 
FEND 
Beginning frequency for using this database 
Ending frequency for using this database
FILENAME 
Path  and  name  of 
information. 
the  database  which  contains  modal
Remarks: 
1. 
If the binary database files are in the runtime directory, this card is not needed 
for the case without partitioning. 
2.  When  the  option  PARTITION  is  active,  the  binary  database  designated  by 
FILENAME is used for the frequency range starting from (and including) FBEG 
and ending at (not including) FEND.
*FREQUENCY_DOMAIN_RANDOM_VIBRATION 
Available options include: 
<BLANK> 
FATIGUE 
Purpose:    Set  random  vibration  control  options.    When  FATIGUE  option  is  used, 
compute fatigue life of structures or parts under random vibration. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MDMIN  MDMAX 
FNMIN 
FNMAX 
RESTRT 
RESTRM 
Type 
Default 
I 
1 
I 
F 
F 
0.0 
  Card 2 
1 
2 
3 
4 
I 
0 
5 
6 
I 
0 
7 
8 
Variable 
DAMPF 
LCDAM 
LCTYP 
DMPMAS DMPSTF  DMPTYP 
Type 
F 
Default 
0.0 
  Card 3 
1 
I 
0 
2 
I 
0 
3 
F 
F 
0.0 
0.0 
4 
5 
I 
0 
6 
7 
8 
Variable 
VAFLAG  METHOD 
UNIT 
UMLT 
VAPSD 
VARMS 
NAPSD 
NCPSD 
Type 
I 
Default 
none 
I 
0 
I 
F 
I 
I 
I 
1 
I
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LDTYP 
IPANELU 
IPANELV 
TEMPER 
LDFLAG 
Type 
I 
I 
I 
F 
Default 
0.0 
I 
0 
Auto PSD Cards.  Include NAPSD cards of this format, one per excitation. 
  Card 5a 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
STYPE 
DOF 
LDPSD 
LDVEL 
LDFLW 
LDSPN 
CID 
Type 
I 
I 
I 
I 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
Cross PSD Cards.  Include NCPSD cards of this format, one per excitation. 
  Card 5b 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LOAD_I 
LOAD_J 
LCTYP2 
LDPSD1 
LDPSD2 
Type 
I 
I 
Default 
I 
I 
I
Fatigue Card.  Additional card for FATIGUE keyword option. 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MFTG 
NFTG 
SNTYPE 
TEXPOS 
STRSF 
INFTG 
Type 
Default 
I 
0 
I 
1 
I 
0 
F 
F 
0.0 
1.0 
I 
0 
S-N Curve Cards.  NFTG additional cards for FATIGUE keyword option.  Each Card 7 
defines one zone for fatigue analysis and the corresponding S-N fatigue curve for that 
zone. 
  Card 7 
1 
2 
3 
4 
Variable 
PID 
LCID 
PTYPE 
LTYPE 
Type 
I 
I 
Default 
I 
0 
I 
0 
5 
A 
F 
6 
B 
F 
7 
8 
STHRES 
SNLIMT 
F 
0. 
I 
0 
Initial  Damage  Card.    INFTG  additional  cards  for  FATIGUE  keyword  option  when 
INFTG > 0. 
  Card 8 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME 
C 
d3ftg 
  VARIABLE   
DESCRIPTION
MDMIN 
The first mode in modal superposition method (optional). 
MDMAX 
The last mode in modal superposition method (optional).
VARIABLE   
FNMIN 
DESCRIPTION
The minimum natural frequency in modal superposition Method
(optional). 
FNMAX 
The maximum natural frequency in modal superposition method
(optional). 
RESTRT 
Restart option. 
EQ.0: A new modal analysis is performed, 
EQ.1: Restart with d3eigv. 
RESTRM 
Restart option when different types of loads are present. 
EQ.0: don’t read the dump file for PSD and RMS, 
EQ.1: read in PSD and RMS values from the dump file and add
them to the values computed in the current load case. 
DAMPF 
LCDAM 
Modal damping coefficient, ζ. 
Load  Curve  ID  defining  mode  dependent  modal  damping
coefficient ζ. 
LCTYP 
Type of load curve defining modal damping coefficient 
EQ.0: Abscissa value defines frequency, 
EQ.1: Abscissa value defines mode number. 
DMPMAS 
Mass proportional damping constant 𝛼, in Rayleigh damping. 
DMPSTF 
Stiffness proportional damping constant 𝛽, in Rayleigh damping. 
DMPTYP 
Type of damping 
EQ.0: modal damping. 
EQ.1: broadband damping.
VARIABLE   
DESCRIPTION
VAFLAG 
Loading type: 
EQ.0: No random vibration analysis. 
EQ.1: Base acceleration. 
EQ.2: Random pressure. 
EQ.3: Plane wave. 
EQ.4: Shock wave. 
EQ.5: Progressive wave. 
EQ.6: Reverberant wave. 
EQ.7: Turbulent boundary layer wave. 
EQ.8: Nodal force. 
METHOD 
Method for modal response analysis. 
EQ.0: method set automatically by LS-DYNA (recommended) 
EQ.1: modal superposition method 
EQ.2: modal acceleration method 
EQ.3: modal truncation augmentation method 
UNIT 
Flag for acceleration unit conversion: 
EQ.0:  use [length unit]/[time unit]2 as unit of acceleration. 
EQ.1:  use g as unit for acceleration, and SI units (Newton, kg,
meter, second, etc.) elsewhere. 
EQ.2:  use g as unit for acceleration, and Engineering units (lbf,
lbf × second2/inch, inch, second, etc.) elsewhere. 
EQ.3:  use  g  as  unit  for  acceleration,  and  units  (kN,  kg,  mm,
ms, GPa, etc.) elsewhere. 
EQ.-1:  use g as unit for acceleration and provide the multiplier
for converting g to [length unit]/[time unit]2. 
UMLT 
Multiplier  for  converting  g  to  [length  unit]/[time  unit]2  (used 
only for UNIT = -1).
VARIABLE   
DESCRIPTION
VAPSD 
Flag for PSD output: 
EQ.0: Absolute PSD output is requested. 
EQ.1: Relative  PSD  output 
is  requested  (used  only  for
VAFLAG = 1) 
VARMS 
Flag for RMS output: 
EQ.0: Absolute RMS output is requested. 
EQ.1: Relative  RMS  output 
is  requested  (used  only  for
VAFLAG = 1) 
NAPSD 
NCPSD 
Number  of  auto  PSD  load  definition.    Card  5a  is  repeated
“NAPSD”  times,  one  for  each  auto  PSD  load  definition.    The
default value is 1. 
Number  of  cross  PSD  load  definition.    Card  5b  is  repeated
“NCPSD”  times,  one  for  each  cross  PSD  load  definition.    The
default value is 0. 
LDTYP 
Excitation load (LDPSD in card 5) type: 
EQ.0: PSD. 
EQ.1: SPL (for plane wave only). 
EQ.2: time history load. 
IPANELU 
Number of strips in U direction (used only for VAFLAG = 5, 6, 7)
IPANELV 
Number of strips in V direction (used only for VAFLAG = 5, 6, 7) 
TEMPER 
Temperature 
LDFLAG 
Type of loading curves. 
EQ.0: Log-Log interpolation (default) 
EQ.1: Semi-Log interpolation 
EQ.2: Linear-Linear interpolation
VARIABLE   
SID 
DESCRIPTION
GE.0: Set ID for the panel exposed to acoustic environment, or
the  nodes  subjected  to  nodal  force  excitation,  or  nodal
acceleration  excitation.    For  VAFLAG = 1,  base  accelera-
tion, leave this as blank 
LT.0:  used to define the cross-PSD.  |SID| is the ID of the load 
cases. 
STYPE 
Flag specifying meaning of SID. 
EQ.0: Node 
EQ.1: Node Set 
EQ.2: Segment Set 
EQ.3: Part 
EQ.4: Part Set 
LT.0:  used  to  define  the  cross-psd.    |STYPE|  is  the  ID  of  the 
load cases. 
DOF 
Applicable  degrees-of-freedom  for  nodal  force  excitation  or  base 
acceleration (DOF = 1, 2, and 3), or wave direction: 
EQ.0: 
translational  movement  in  direction  given  by  vector
VID. 
EQ.±1:  x-translational degree-of-freedom (positive or negative)
EQ.±2:  y-translational degree-of-freedom (positive or negative)
EQ.±3:  z-translational degree-of-freedom (positive or negative)
LDPSD 
Load curve for PSD, SPL, or time history excitation. 
LDVEL 
Load curve for phase velocity. 
LDFLW 
Load curve for exponential decay for TBL in flow-wise direction 
LDSPN 
Load curve for exponential decay for TBL in span-wise direction 
CID/VID 
Coordinate system ID for defining wave direction, see *DEFINE_-
COORDINATE_SYSTEM; or Vector ID for defining load direction 
for nodal force, or base excitation, see *DEFINE_VECTOR. 
LOAD_I 
ID of load i for cross PSD. 
LOAD_J 
ID of load j for cross PSD.
VARIABLE   
LCTYP2 
DESCRIPTION
Type  of  load  curves  (LDPSD1  and  LDPSD2)  for  defining  cross
PSD: 
EQ.0:  LDPSD1  defines  real  part  and  LDPSD2  defines
imaginary part 
EQ.1:  LDPSD1 defines magnitude and LDPSD2 defines phase
angle 
LDPSD1 
Load curve for real part or magnitude of cross PSD 
LDPSD2 
Load curve for imaginary part or phase angle of cross PSD 
MFTG 
Method for random fatigue analysis (for option_FATIGUE). 
EQ.0: no fatigue analysis, 
EQ.1: Steinberg’s three-band method, 
EQ.2: Dirlik method, 
EQ.3: Narrow band method, 
EQ.4: Wirsching method, 
EQ.5: Chaudhury and Dover method, 
EQ.6: Tunna method, 
EQ.7: Hancock method. 
NFTG 
Field specifying the number of S - N curves to be defined. 
GE.0: Number  of  S - N  curves  defined  by  card  6.    Card  6  is 
repeated  “NFTG”  number  of  times,  one  for  each  S - N 
fatigue curve definition.  The default value is 1. 
EQ.-999:  S - N curves are defined through *MAT_ADD_FA-
TIGUE. 
If the option FATIGUE is not used, ignore this parameter. 
SNTYPE 
Stress type of S - N curve in fatigue analysis. 
EQ.0:  von-mises stress 
EQ.1:  maximum principal stress (not implemented) 
EQ.2:  maximum shear stress (not implemented) 
EQ.-n:  The nth stress component. 
TEXPOS 
Exposure time (used if option FATIGUE is used)
VARIABLE   
STRSF 
DESCRIPTION
Stress  scale  factor  to  accommodate  different  ordinates  in  S - N 
curve. 
EQ.1: used  if  the  ordinate  in  S - N  curve  is  stress  range 
(default) 
EQ.2: used if the ordinate in S - N curve is stress amplitude 
INFTG 
Flag for including initial damage ratio. 
EQ.0: no initial damage ratio, 
GT.0:  read existing d3ftg files to get initial damage ratio.  When 
INFTG > 1,  it  means  that  the  initial  damage  ratio  comes
from  multiple  loading  cases  (correspondingly,  multiple
binary  databases,  defined  by  Card  7).    The  value  of
INFTG should be ≤ 10.  
PID 
Part ID, or Part Set ID, or Element (solid, shell, beam, thick shell)
Set ID.  
LCID 
S - N fatigue curve ID for the current Part or Part Set. 
GT.0:  S - N fatigue curve ID 
EQ.-1:  S - N fatigue curve uses equation 𝑁𝑆𝑏 = 𝑎 
EQ.-2:  S - N fatigue curve uses equation log(𝑆) = 𝑎 − 𝑏 log(𝑁) 
EQ.-3:  S - N fatigue curve uses equation 𝑆 = 𝑎 𝑁𝑏 
PTYPE 
Type of PID. 
EQ.0: Part (default) 
EQ.1: Part Set 
EQ.2: SET_SOLID 
EQ.3: SET_BEAM 
EQ.4: SET_SHELL 
EQ.5: SET_TSHELL 
LTYPE 
Type of LCID. 
EQ.0: Semi-log interpolation (default) 
EQ.1: Log-Log interpolation 
EQ.2:  Linear-Linear interpolation
VARIABLE   
DESCRIPTION
A 
B 
Material parameter 𝑎 in S - N fatigue equation. 
Material parameter 𝑏 in S - N fatigue equation. 
STHRES 
Fatigue threshold (applicable only if LCID < 0). 
SNLIMT 
If LCID > 0 
Flag setting algorithm used when  stress is lower than the lowest
stress  on  S - N  curve  (if  LCID > 0),  or  lower  than  STHRES  (if 
LCID < 0). 
EQ.0: use the life at the last point on S - N curve 
EQ.1: extrapolation  from  the  last  two  points  on  S - N  curve 
(only applicable if LCID > 0) 
EQ.2: infinity. 
If LCID < 0 
Flag setting algorithm used when stress is lower STHRES 
EQ.0: use the life at STHRES 
EQ.1: Ingnored.  only applicable for LCID > 0 
EQ.2: infinity. 
FILENAME 
Path  and  name  of  existing  binary  database 
information. 
for 
fatigue
Remarks: 
1.  Historical  Background.    This  command  evaluates  the  structural  random 
vibration  response  due  to  aero  acoustic  loads,  base  excitation,  or  nodal  force.  
This capability originated in Boeing’s in-house code N-FEARA, which is a  NI-
KE3D-based Finite Element tool for performing structural analysis  with vibro-
acoustic loads.  The main developer of N-FEARA is Mostafa Rassaian from the 
Boeing Company. 
2.  Fatigue.    To  run  this  option,  it  is  required  that  MSTRES = 1  in  the  keyword 
*CONTROL_IMPLICIT_EIGENVALUE.  This is because the fatigue analysis is 
depends on stresses. 
3. 
IPANEL.  The number of strips the in U and V direction are used to group the 
elements and thereby reduce the number integration domains reducing compu-
tational expense.  This option is only available for VAFLAG = 5, 6, and 7.
4.  Restarting.   Restart  option  RESTRT = 1  is  used  when  mode  analysis  has  been 
done previously.  In this case, LS-DYNA skips modal analysis and reads in the 
d3eigv files from the prior execution.  For RESTMD = 1, always use MDMIN = 1 
and set MDMAX to the number of modes in the previous run (this can be found 
in  the  ASCII  file  eigout,  or  it  can  be  extracted  from  the  d3eigv  files  using  LS-
PrePost). 
5.  Accumulated  Fatigue.    The  fatigue  damage  ratio  can  be  accumulated  over 
multiple  load  cases  by  setting  INFTG = 1.    This  is  useful  when  a  structure  is 
subjected to multiple independent random vibrations.  LS-DYNA calculates the 
total damage ratio by adding the damage ratio from the current calculation to 
the  damage  ratio  of  the  previous  calculation  which  are  stored  in  the  previous 
calculation’s fatigue database (d3ftg by default).  The previous d3ftg file will be 
overwritten by the new one, if it is in the same directory. 
6.  Automatic  Method  Selection.    If  METHOD = 0,  LS-DYNA  uses  modal 
superposition method for cases (VAFLAG) 4, 5, 6, 7; For cases 1, 2, 3 and 8, LS-
DYNA  uses  modal  superposition  method  when  preload  condition  is  present 
and uses modal acceleration method when preload condition is not present. 
7.  Units.  In a set of consistent units, the unit for acceleration is defined as 
1  (acceleration  unit) =
1(length  unit)
[1(time  unit)]2 
Some users in industry prefer to use g (acceleration due to gravity) as the unit 
for acceleration.  For example, 
1g = 9.81
s2 = 386.089
inch
s2  
If the input and output use g as the unit for acceleration, select UNIT = 1, 2, or 
3. 
If UNIT = 3, a multiplier (UMLT) for converting g to [length unit]/[time unit]2 
is needed and it is defined by 
1g = UMLT ×
[length unit]
[time unit]2  
For more information about the consistent units, see GS.21 (GETTING START-
ED). 
8.  Restrictions on Load Curves.  The load curves LDPSD, LDVEL, LDFLW, and 
LDSPN must all be defined using the same number of points.  The number of 
points  in  the  load  curve  LDDAMP  can  be  different  from  those  for  LDPSD, 
LDVEL, LDFLW, and LDSPN.
9.  Wave direction.  Wave direction is determined DOF and CID/VID.  CID/VID 
represents  a  local  U-V-W  coordinate  system  for  defining  acoustic  wave  direc-
tion,  only  partially  correlated  waves  (VAFLAG=5,  6,  7)  need  this  local  coordi-
nate system.  For nodal force, base excitation, plane wave or random pressure, 
CID represents a vector ID defining the load direction (DOF = ±4). 
10.  Stress  /  Strain  computation.  To  get  stress  results  (PSD  and  RMS)  from 
random  vibration  analysis,  MSTRES  field  of  the  *CONTROL_IMPLICIT_-
EIGENVALUE  keyword  should  be  set  to  1.    To  get  strain  results  (PSD  and 
RMS) the STRFLG field of *DATABASE_EXTENT_BINARY should be set to 1.   
To  get  stress  component  results  for  beam  elements  (which  are  not  based  on 
resultant  formulation),  the  BEAMIP  field  of  *DATABASE_EXTENT_BINARY 
should be set greater than 0. 
11.  Binary  plot  databases.    PSD  and  RMS  results  are  given  for  all  nodes  and 
elements.   PSD results are written in binary to a file named d3psd.  Similarly, 
RMS  results  are  written  in  binary  to  a  file  named  d3rms.    See  the  keyword 
*DATABASE_FREQUENCY_BINARY_{OPTION} for more details. 
12.  ASCII  Output  for  Displacement.    Displacement,  velocity,  and  acceleration 
PSD  results  are  output  into  ASCII  file  nodout_psd.    The  set  nodes  for  which 
data  is  written  to  nodout_psd  is  specified  with  the  *DATABASE_HISTORY_-
NODE keyword. 
13.  ASCII Output for Stress.  Stress PSD results are output into ASCII file elout_
psd.  The set of solid, beam, shell, and thick shell elements to be written to the 
elout_psd file are specified with the following keywords: *DATABASE_HISTO-
RY_SOLID,  *DATABASE_HISTORY_BEAM,    *DATABASE_HISTORY_SHELL,  
*DATABASE_HISTORY_TSHELL. 
14.  Cross  PSD.    The  cross  PSD  can  be  defined  as  complex  variables  to  consider 
phase  difference.    In  that  case,  two  curves  are  needed  to  define  the  cross  PSD 
(LCPSD1  and  LCPSD2).    Two  load  IDs  are  needed  to  define  the  cross  PSD 
(LOAD_I  and  LOAD_J).    They  are  simply  the  ordering  numbers  by  which  the 
auto  PSDs  are  defined.    For  example,  the  first  Card  5a  defines  load  1  and  the 
second  Card  5a  defines  the  load  2.    No  cross  PSD  is  required  if  two  loads  are 
uncorrelated.    Cross  PSD  for  any  pair  of  two  correlated  loads  is  defined  only 
once  –  from  lower  load  ID  to  higher  load  ID  (e.g.    1->2,  1->3,  2->3,  …).    The 
cross  PSD  from  higher  load  ID  to  lower  load  ID  (e.g.    2->1,  3->1,  3->2,  …)  is 
added by LS-DYNA automatically by using the relationship 
̅̅̅̅̅̅̅̅̅ 
𝐺𝑗𝑖 = 𝐺𝚤𝚥
where 𝐺𝑖𝑗 is the cross PSD from load i to load j, and ̅̅̅̅̅̅̅ represents the complex 
conjugate.
15.  Cross  Correlation.    Cross  correlation  can  be  defined  only  for  same  type  of 
excitations (e.g.  nodal force, random pressure).  Correlation between different 
types of excitations is not allowed 
16.  Output  for  Fatigue  Data.    When  the  FATIGUE  option  is  used,  a  binary  plot 
file, d3ftg, is written.  5 results are included in d3ftg: 
Result 1.  Cumulative damage ratio 
Result 2.  Expected fatigue life 
Result 3.  Zero-crossing frequency 
Result 4.  Peak-crossing frequency 
Result 5.  Irregularity factor 
These results are given as element variables.  Irregularity factor is a real number 
from  0  to  1.    A  sine  wave  has  irregularity  factor  as  1,  while  white  noise  has 
irregularity factor as 0.  The lower the irregularity factor, the closer the process 
is to the broad band case. 
17.  Stress  Threshold  for  Fatigue.    In  some  materials,  the S−N  curve  flattens  out 
eventually,  so  that  below  a  certain  threshold  stress  STHRES  failure  does  not 
occur no matter how long the loads are cycled.  SNLIMT can be set to 2 in this 
case;  For  other  materials,  such  as  aluminum,  no  threshold  stress  exists  and 
SNLIMT should be set to 0 or 1 for added level of safety. 
18.  Restriction on Fatigue Cards.  When the FATIGUE option is used, all fatigue 
cards (Card 6) must be of the same PTYPE (PART or SET of ELEMENTS). 
19.  Format for S - N Curves.  S - N curves can be defined by *DEFINE_CURVE, or 
for LCID<0 by 
when LCID = -1 or for LCID = -2 
𝑁𝑆𝑏 = 𝑎 
or for LCID = -3 
log(𝑆) = 𝑎 − 𝑏 log(𝑁) 
𝑆 = 𝑎 𝑁𝑏 
where N is the number of cycles for fatigue failure and S is the stress amplitude.  
Please  note  that  the  two  equations  can  be  converted  to  each  other,  with  some 
minor manipulation on the constants a and b.
References: 
Mostafa  Rassaian,  Jung-Chuan  Lee,  N-FEARA  –  NIKE3D-based  FE  tool  for  structural 
analysis of vibro-acoustic loads, Boeing report, 9350N-GKY-02-036, December 5, 2003.
*FREQUENCY_DOMAIN_RESPONSE_SPECTRUM 
Purpose:    perform  response  spectrum  computation  to  obtain  the  peak  response  of  a 
structure. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MDMIN  MDMAX 
FNMIN 
FNMAX 
RESTRT  MCOMB 
Type 
Default 
I 
1 
I 
F 
F 
0.0 
  Card 2 
1 
2 
3 
4 
I 
0 
5 
I 
0 
6 
7 
8 
Variable 
DAMPF 
LCDAMP 
LDTYP 
DMPMAS DMPSTF 
Type 
F 
I 
Default 
none 
none 
I 
0 
F 
F 
0.0 
0.0 
Card  3  can  be  repeated  if  2  or  more  input  spectra  exist  (multiple-point  response 
spectrum) 
  Card 3 
1 
2 
3 
Variable 
LCTYP 
DOF 
LC/TBID 
Type 
I 
I 
I 
Default 
4 
SF 
F 
1.0 
5 
6 
7 
8 
VID 
LNID 
LNTYP 
INFLAG 
I 
I 
I 
I 
0 
  VARIABLE   
DESCRIPTION
MDMIN 
MDMAX 
The first mode in modal superposition method (optional). 
The last mode in modal superposition method (optional).
FNMIN 
FNMAX 
The minimum natural frequency in modal superposition method
(optional). 
The maximum natural frequency in modal superposition method
(optional). 
RESTRT 
Restart option 
EQ.0: A new run including modal analysis, 
EQ.1: Restart with d3eigv family files created elsewhere. 
MCOMB 
Method for combination of modes: 
EQ.0: SRSS method, 
EQ.1: NRC Grouping method, 
EQ.2: Complete Quadratic Combination method (CQC), 
EQ.3: Double  Sum  method  based  on  Rosenblueth-Elorduy 
coefficient, 
EQ.4: NRL-SUM method, 
EQ.5: Double  Sum  method  based  on  Gupta-Cordero 
coefficient, 
EQ.6: Double  Sum  method  based  on  modified  Gupta-Cordero 
coefficient, 
EQ.7: Rosenblueth method. 
DAMPF 
Modal damping ratio, ζ. 
LCDAMP 
Load Curve ID for defining frequency dependent modal damping 
ratio ζ. 
LDTYP 
Type of load curve for LCDAMP 
EQ.0: Abscissa value defines frequency, 
EQ.1: Abscissa value defines mode number. 
DMPMAS 
Mass proportional damping constant α, in Rayleigh damping. 
DMPSTF 
Stiffness proportional damping constant β, in Rayleigh damping.
LCTYP 
Load curve type for defining the input spectrum. 
EQ.0:  base velocity, 
EQ.1:  base acceleration, 
EQ.2:  base displacement, 
EQ.3:  nodal force, 
EQ.4:  pressure, 
EQ.10:  base velocity time history, 
EQ.11:  base acceleration time history, 
EQ.12:  base displacement time history. 
DOF 
Applicable degrees-of-freedom for excitation input: 
EQ.1: x-translational degree-of-freedom, 
EQ.2: y-translational degree-of-freedom, 
EQ.3: z-translational degree-of-freedom, 
EQ.4: translational movement in direction given by vector VID.
Load  curve  or  table  ID,  see  *DEFINE_TABLE,  defining  the 
response spectrum for frequencies.  If the table definition is used
a family of curves are defined for discrete critical damping ratios.
Scale factor for the input load spectrum. 
Vector ID for DOF values of 4. 
Node ID, or node set ID, or segment set ID where the excitation is
applied.    If  the  input  load  is  given  as  base  excitation  spectrum,
LNID = 0 
LC/TBID 
SF 
VID 
LNID 
LNTYP 
Set type for LNID: 
EQ.1: Node, see *NODE, 
EQ.2: Node set, see *SET_NODE, 
EQ.3: Segment set, see *SET_SEGMENT, 
EQ.4: Part, see *PART, 
EQ.5: Part set, see *SET_PART.
INFLAG 
Frequency interpolation option 
EQ.0: Logarithmic interpolation, 
EQ.1: Semi-logarithmic interpolation. 
EQ.2: Linear interpolation. 
Remarks: 
1.  This  command  uses  modal  superposition  method  to  evaluate  the  maximum 
response of a structure subjected to input response spectrum load, such as the 
acceleration spectrum load in earthquake engineering. 
2.  Modal analysis has to be performed preceding the response spectrum analysis.  
Thus  the  keywords  *CONTROL_IMPLICIT_GENERAL  and  *CONTROL_IM-
PLICIT_EIGENVALUE are expected in the input file. 
3.  MDMIN, MDMAX, FNMIN and FNMAX should be set appropriately to cover 
all the natural modes inside the input spectrum. 
4.  To  include  stress  results,  modal  stress  computation  has  to  be  requested  in 
*CONTROL_IMPLICIT_EIGENVALUE (set MSTRES = 1). 
5.  For base excitation cases, user can choose relative values or absolute values for 
displacement, velocity and acceleration results output. 
6.  RESTRT = 1 enables a fast restart run based on d3eigv family files generated in 
last  run  or  elsewhere.    LS-DYNA  reads  d3eigv  family  files  to  get  the  natural 
vibration frequencies and mode shapes.  If the d3eigv family files are located in 
a directory other than the working directory, the directory must be specified in 
*FREQUENCY_DOMAIN_PATH. 
7.  For  Double  Sum  method  (MCOMB = 3),  earthquake  duration  time  is  given  by 
ENDTIM in the keyword *CONTROL_TERMINATION. 
8.  Three  interpolation  options  are  available  for  frequency  interpolation  when 
reading response spectrum values  
a)  When INFLAG = 0 (default), logarithmic interpolation is used, e.g. 
log𝑦 − log𝑦1
log𝑥 − log𝑥1
=
log𝑦2 − log𝑦1
log𝑥2 − log𝑥1
b)  When INFLAG = 1, semi-logarithmic interpolation is used, e.g. 
log𝑦 − log𝑦1
𝑥 − 𝑥1
=
log𝑦2 − log𝑦1
𝑥2 − 𝑥1
c)  When INFLAG = 2, linear interpolation is used, e.g. 
𝑦 − 𝑦1
𝑥 − 𝑥1
𝑦2 − 𝑦1
𝑥2 − 𝑥1
=
9.  Linear interpolation is used for interpolation with respect to damping ratios.
*FREQUENCY_DOMAIN_SSD_{OPTION} 
Available options include: 
FATIGUE 
ERP 
Purpose:  Compute steady state dynamic response due to given spectrum of harmonic 
excitations.  
When the FATIGUE option is applied LS-DYNA also calculates the cumulative fatigue 
damage ratio.  When the ERP option is applied LS-DYNA also calculates the Equivalent 
Radiated Power (ERP) due to vibration. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MDMIN  MDMAX 
FNMIN 
FNMAX 
RESTMD  RESTDP 
LCFLAG 
RELATV 
Type 
Default 
I 
1 
I 
F 
F 
0.0 
  Card 2 
1 
2 
3 
4 
I 
0 
5 
I 
0 
6 
I 
0 
7 
I 
0 
8 
Variable 
DAMPF 
LCDAM 
LCTYP 
DMPMAS DMPSTF  DMPFLG 
Type 
F 
Default 
0.0 
  Card 3 
1 
I 
0 
2 
I 
0 
3 
F 
F 
0.0 
0.0 
4 
5 
I 
0 
6 
7 
8 
Variable 
Type 
Default 
MEMORY
NERP 
STRTYP 
NOUT 
NOTYP 
NOVA 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I
ERP Card.  This card is read only when the ERP option is active. 
  Card 4a 
Variable 
1 
RO 
Type 
F 
2 
C 
F 
3 
4 
5 
6 
7 
8 
ERPRLF 
ERPREF 
F 
F 
Default 
none 
none 
1.0 
0.0 
ERP Part Cards.  This card is read NERP times.  Since NERP defaults to zero this card 
is, by default not read, and, furthermore, it is not read unless the ERP option is active. 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
PTYP 
Type 
I 
Default 
none 
I 
0 
Excitation Loads.  Repeat Card 4 if multiple excitation loads are present.  
  Card 4 
1 
2 
3 
4 
5 
6 
7 
Variable 
NID 
NTYP 
DOF 
VAD 
LC1 
LC2 
LC3 
Type 
I 
Default 
none 
I 
0 
I 
I 
I 
I 
none 
none 
none 
none 
I 
0 
8 
VID 
I 
0 
  VARIABLE   
DESCRIPTION
MDMIN 
The first mode in modal superposition method (optional). 
MDMAX 
The last mode in modal superposition method (optional). 
FNMIN 
The minimum natural frequency in modal superposition method
(optional).
VARIABLE   
FNMAX 
DESCRIPTION
The maximum natural frequency in modal superposition method
(optional). 
RESTMD 
Restart option: 
EQ.0: A new modal analysis is performed, 
EQ.1: Restart with d3eigv. 
RESTDP 
Restart option: 
EQ.0: A new run without dumpssd, 
EQ.1: Restart with dumpssd. 
LCFLAG 
Load Curve definition flag. 
EQ.0: load curves are given as amplitude / phase angle, 
EQ.1: load curves are given as real / imaginary components. 
RELATV 
Flag for displacement, velocity and acceleration results: 
EQ.0: absolute values are requested, 
EQ.1: relative values are requested (for VAD = 2, 3 and 4 only).
DAMPF 
LCDAM 
Modal damping coefficient, ζ. 
Load  Curve  ID  defining  mode  dependent  modal  damping
coefficient ζ. 
LCTYP 
Type of load curve defining modal damping coefficient. 
EQ.0: Abscissa value defines frequency, 
EQ.1: Abscissa value defines mode number. 
DMPMAS 
Mass proportional damping constant 𝛼, in Rayleigh damping. 
DMPSTF 
Stiffness proportional damping constant 𝛽, in Rayleigh damping 
DMPFLG 
Damping flag: 
EQ.0: use modal damping coefficient 𝜁 , defined by DAMPF, or 
LCDAM,  or  Rayleigh  damping  defined  by  DMPMAS 
and DMPSTF in this card. 
EQ.1: use  damping  defined  by  *DAMPING_PART_MASS  and
*DAMPING_PART_STIFFNESS.
VARIABLE   
DESCRIPTION
MEMORY 
Memory flag: 
EQ.0: modal  superposition  will  be  performed  in-core.    This 
option runs faster. 
EQ.1: modal superposition will be performed out-of-core.  This 
is needed for some large scale problems that cannot fit in
main memory.  This method incurs a performance penal-
ty associated with disk speed. 
NERP 
Number of ERP panels. 
STRTYP 
Stress used in fatigue analysis: 
EQ.0: Von Mises stress, 
EQ.1: Maximum principal stress, 
EQ.2: Maximum shear stress. 
NOUT 
Part, part set, segment set, or node set ID for response output (use
with acoustic computation).  See NOTYP below. 
NOTYP 
Type of NOUT: 
EQ.0:  part set ID (not implemented), 
EQ.1:  part ID (not implemented), 
EQ.2:  segment set ID, 
EQ.3:  node set ID, 
EQ.-2:  segment  set  ID  which  mismatches  with  acoustic
boundary nodes.  Mapping of velocity or acceleration to
the acoustic boundary nodes is performed. 
NOVA 
Response output type. 
EQ.0: velocity, 
EQ.1: acceleration. 
RO 
C 
Fluid density. 
Sound speed of the fluid. 
ERPRLF 
ERP radiation loss factor. 
ERPREF 
ERP  reference  value.    This  is  used  to  convert  the  absolute  ERP
value to ERP in decibels (dB).
VARIABLE   
PID 
DESCRIPTION
Part, part set, or segment set ID for ERP computation.  See PTYP
below. 
PTYP 
Type of PID: 
EQ.0:  part ID, 
EQ.1:  part set ID, 
EQ.2:  segment set ID. 
NID 
Node, node set, or segment set ID for excitation input.  See NTYP
below. 
NTYP 
Type of NID. 
EQ.0: node ID, 
EQ.1: node set ID, 
EQ.2: segment set ID. 
DOF 
Applicable  degrees-of-freedom  for  excitation  input  (ignored  if 
VAD = 1). 
EQ.1: 𝑥-translational degree-of-freedom, 
EQ.2: 𝑦-translational degree-of-freedom, 
EQ.3: 𝑧-translational degree-of-freedom, 
EQ.4: translational movement in direction given by vector VID.
VAD 
Excitation input type: 
EQ.0: nodal force, 
EQ.1: pressure, 
EQ.2: base velocity, 
EQ.3: base acceleration, 
EQ.4: base displacement, 
EQ.5: enforced velocity by large mass method ,
EQ.6: enforced acceleration by large mass method , 
EQ.7: enforced  displacement  by  large  mass  method  .
VARIABLE   
DESCRIPTION
Load  Curve  ID  defining  amplitude  (LCFLAG = 0)  or  real  (in-
phase) part (LCFLAG = 1) of load as a function of frequency. 
Load Curve ID defining phase angle (LCFLAG = 0) or imaginary 
(out-phase) part (LCFLAG = 1) of load as a function of frequency.
Load  Curve  ID  defining  load  duration  for  each  frequency.    This
parameter is optional and is only needed for fatigue analysis. 
Vector  ID  for  DOF = 4  for  excitation  input,  see  *DEFINE_VEC-
TOR. 
LC1 
LC2 
LC3 
VID 
Remarks: 
1.  This  command  computes  steady  state  dynamic  response  due  to  harmonic 
excitation spectrum by modal superposition method. 
2.  Natural  frequencies  and  mode  shapes  are  needed  for  running  the  modal 
superposition  method.    Thus,  the  keyword  *CONTROL_IMPLICIT_EIGEN-
VALUE must be included in input. 
3.  MDMIN/MDMAX and FNMIN/FNMAX together determine which modes are 
used in modal superposition method.  The first mode must have a mode num-
ber ≥ MDMIN, and frequency ≥ FNMIN; The last mode must have mode num-
ber  ≤  MDMAX,  and  frequency  ≤  FNMAX.    When  MDMAX  or  FNMAX  is  not 
given, the last mode in modal superposition method is the last mode available 
in FILENM. 
4.  Restart option RESTMD = 1 is used if mode analysis has been done previously.  
In  this  case,  LS-DYNA  skips  modal  analysis  and  reads  in  d3eigv  family  files 
generated  previously. 
  For  RESTMD = 1,  always  use  MDMIN = 1  and 
MDMAX = number  of  modes  given  by  modal  analysis  (can  be  found  from 
ASCII file eigout, or from d3eigv files using LS-PREPOST). 
5.  Restart  option  RESTDP = 1  is  used  if  user  wants  to  add  contribution  of 
additional modes to previous SSD results.  In this case, LS-DYNA reads in bina-
ry dump file dumpssd which contains previous SSD results and adds contribu-
tion from new modes.  For RESTDP = 1, the new modal analysis (RESTMD = 0) 
or the d3eigv family files created elsewhere (RESTMD = 1) should  exclude the 
modes used in previous SSD computation.  This can be done by setting LFLAG 
(and  RFLAG,  if  necessary),  and  setting  a  nonzero  LFTEND  (and  RHTEND)  in 
*CONTROL_IMPLICIT_EIGENVALUE.    The  RESTDP  option  can  also  be  used
if  the  frequency  range  for  modal  analysis  is  divided  into  segments  and  modal 
analysis is performed for each frequency range separately. 
6.  Sometimes  customers  would  like  to  add  some  acoustic  field  nodes  and  run 
BEM/FEM acoustic computation after SSD.  The RESTMD and RESTDP options 
still  work even  if the number  of  nodes  may  get  changed  after  previous  modal 
analysis, provided that the IDs of the old nodes are not changed. 
7.  Damping can be prescribed in several ways: 
a)  To  use  a  constant  modal  damping  coefficient   for  all  the  modes,  define 
DAMPF only.  LCDMP, LCTYP, DMPMAS and DMPSTF are ignored. 
b)  To use mode dependent modal damping, define a load curve (*DEFINE_-
CURVE)  and  specify  that  if  the  abscissa  value  defines  the  frequency  or 
mode number by LCTYP.  DMPMAS and DMPSTF are ignored. 
c)  To use Rayleigh damping, define DMPMAS (𝛼) and DMPSTF (𝛽) and keep 
DAMPF  as  0.0,  and  keep  LCDMP,  LCTYP  as  0.    The  damping  matrix  in 
Rayleigh damping is defined as 𝐂 = 𝐌 + 𝐊, where, 𝐂, 𝐌 and 𝐊 are the 
damping, mass and stiffness matrices respectively. 
8.  NOUT and NOTYP are used to define the nodes where velocity or acceleration 
are requested to be written to a binary file “bin_ssd” or other filename defined 
by  “bem=filename”   in command line.  The velocity or acceleration data in this file can be used 
by  BEM  or  FEM  acoustic  solver  to  perform a  vibro-acoustic  analysis.    If  struc-
ture nodes and acoustic boundary nodes are mismatched, the option NOTYP = 
-2 can  be used.  The velocity or acceleration data given at a structure segment 
set NOUT is mapped to acoustic boundary nodes. 
9.  For  base  velocity,  base  acceleration  or  base  displacement  (VAD = 2,  3  or  4) 
excitations, the parameters NID, NTYP are not used and can be blank.  The base 
velocity, base acceleration and base displacement cases are treated by applying 
inertia force to the structure. 
10.  For the cases with enforced motion excitation such as nodal velocity, accelera-
tion, or displacement) the large mass method can be used to compute the SSD 
results.  The excitation input can be given as enforced motion curves (VAD = 5, 
6, 7).  To use the large mass method, the user need to attach a large mass to the 
nodes  where  the  enforced  motion  is  applied  by  using  the  keyword  *ELE-
MENT_MASS_{OPTION},  and  report  the  large  mass  per  node  (MPN)  in  the 
keyword *CONTROL_FREQUENCY_DOMAIN.  For more details, please refer 
to *CONTROL_FREQUENCY_DOMAIN.
11.  Displacement,  velocity  and  acceleration  results  are  output  into  ASCII  file 
NODOUT_SSD.  The nodes to be output to NODOUT_SSD are specified by card 
*DATABASE_HISTORY_NODE. 
12.  Stress  results  are  output  into  ASCII  file  ELOUT_SSD.    The  solid,  beam,  shell 
and  thick  shell  elements  to  be  output  to  ELOUT_SSD  are  specified  by  the  fol-
lowing cards: 
*DATABASE_HISTORY_SOLID_{OPTION} 
*DATABASE_HISTORY_BEAM_{OPTION} 
*DATABASE_HISTORY_SHELL_{OPTION} 
*DATABASE_HISTORY_TSHELL_{OPTION} 
13.  The phase angle is given in range (-180°, 180°]. 
14.  When the FATIGUE option is present, the cumulative fatigue damage ratio due 
to the harmonic vibration is computed and saved in binary plot database d3ftg.  
The *MATERIAL_ADD_FATIGUE keyword is needed to define the S-N fatigue 
curve for each material.
Purpose:    Define  hourglass  and  bulk  viscosity  properties  which  are  referenced  via 
HGID in the *PART command.  Properties specified here, when invoked for a particular 
part,  override  those  in  *CONTROL_HOURGLASS  and  *CONTROL_BULK_VISCOSI-
TY. 
An  additional  option  TITLE  may  be  appended  to  *HOURGLASS  keywords.    If  this 
option is used then an additional line is read for each section in 80a format which can be 
used  to  describe  the  section.    At  present  LS-DYNA  does  not  make  use  of  the  title.  
Inclusion of titles gives greater clarity to input decks. 
  Card 1 
1 
2 
3 
4 
Variable 
HGID 
IHQ 
QM 
IBQ 
Type 
I/A 
I 
F 
I 
5 
Q1 
F 
6 
7 
8 
Q2 
QB, VDC 
QW 
F 
F 
F 
Default 
0 
.10 
1.5 
0.06 
QM, 0. 
QM 
Remark 
1,6 
2 ,4, 7 
3 
3 
5 
5 
  VARIABLE   
HGID 
DESCRIPTION
Hourglass ID.  A unique number or label must be specified.  This
ID is referenced by HGID in the *PART command.
IHQ 
DESCRIPTION
Hourglass  control  type.    For  solid  elements  six  options  are
available.    For  quadrilateral  shell  and  membrane  elements  the
hourglass  control  is  based  on  the  formulation  of  Belytschko  and
Tsay, i.e., options 1-3 are identical, and options 4-5 are identical: 
EQ.0:  see remark 9, 
EQ.1:  standard LS-DYNA viscous form, 
EQ.2:  Flanagan-Belytschko viscous form, 
EQ.3:  Flanagan-Belytschko  viscous  form  with  exact  volume 
integration for solid elements, 
EQ.4:  Flanagan-Belytschko stiffness form, 
EQ.5:  Flanagan-Belytschko  stiffness  form  with  exact  volume 
integration for solid elements. 
EQ.6:  Belytschko-Bindeman 
co-
rotational  stiffness  form  for  2D  and  3D  solid  elements 
only. 
[1993]  assumed 
strain 
EQ.7:  Linear  total  strain  form  of  type  6  hourglass  control.
. 
EQ.8:  Activates  full  projection  warping  stiffness  for  shell
formulations  16  and  -16,  and  is  the  default  for  these 
formulations.    A  speed  penalty  of  25%  is  common  for 
this option. 
EQ.9:  Puso [2000] enhanced assumed strain stiffness form for
3D hexahedral elements. 
EQ.10:  Cosserat  Point  Element  (CPE)  developed  by  Jabareen
and Rubin [2008] and Jabareen et.al.  [2013], see *CON-
TROL_HOURGLASS. 
A  discussion  of  the  viscous  and  stiffness  hourglass  control  for
shell elements follows at the end of this section..
Hourglass coefficient.  Values of QM that exceed 0.15 may cause
instabilities for brick elements used with forms IHG = 0 to 5 and 
all  the  IHG  forms  applicable  to  shell  elements.    The  stiffness
forms can stiffen the response especially if deformations are large
and  therefore  should  be  used  with  care.    For  the  shell  and
membrane  elements  QM  is  taken  as  the  membrane  hourglass
coefficient,  the  bending  as  QB,  and  warping  as  QW.    These
coefficients  can  be  specified 
independently,  but  generally,
QM = QB = QW, is adequate.  For type 6 solid element hourglass
control, see remark 4 below.  For hourglass type 9, see Remark 8.  
Not  used.    Bulk  viscosity  is  always  on  for  solids.    Bulk  viscosity
for  beams  and  shells  can  only  be  turned  on  using  the  variable
TYPE 
the 
*CONTROL_BULK_VISCOSITY; 
coefficients can be set using Q1 and Q2 below. 
however, 
in 
Quadratic bulk viscosity coefficient. 
Linear bulk viscosity coefficient. 
Hourglass  coefficient  for  shell  bending.    The  default:  QB = QM. 
. 
Viscous damping coefficient for types 6 and 7 hourglass control. 
Hourglass coefficient for shell warping.  The default: QB = QW. 
  VARIABLE   
QM 
IBQ 
Q1 
Q2 
QB 
VDC 
QW 
Remarks: 
1.  Viscous  hourglass  control  is  recommended  for  problems  deforming  with  high 
velocities.  Stiffness control is often preferable for lower velocities, especially if 
the  number  of  time  steps  are  large.    For  solid  elements  the  exact  volume  inte-
gration provides some advantage for highly distorted elements. 
2.  For  automotive  crash  the  stiffness  form  of  the  hourglass  control  with  a 
coefficient of 0.05 is preferred by many users. 
3.  Bulk  viscosity  is  necessary  to  propagate  shock  waves  in  solid  materials.  
Generally, the default values are okay except in problems where pressures are 
very  high,  larger  values  may  be  desirable.    In  low  density  foams,  it  may  be 
necessary to reduce the viscosity values since the viscous stress can be signifi-
cant.  It is not advisable to reduce it by more than an order of magnitude.
constants and an assumed strain field, it produces accurate coarse mesh bend-
ing  results  for  elastic  material  when  QM = 1.0.    For  plasticity  models  with  a 
yield  stress  tangent  modulus  that  is  much  smaller  than  the  elastic  modulus,  a 
smaller  value  of  QM  (0.001  to  0.1)  may  produce  better  results.    For  foam  or 
rubber  models,  larger  values  (0.5  to  1.0)  may  work  better.    For  any  material, 
keep in mind that the stiffness is based on the elastic constants, so if the materi-
al softens, a QM value smaller than 1.0 may work better.  For anisotropic mate-
rials, an average of the elastic constants is used.  For fluids modeled with null 
material, type 6 hourglass control is viscous and is scaled to the viscosity coeffi-
cient of the material . 
5. 
In part, the computational efficiency of the Belytschko-Lin-Tsay and the under 
integrated  Hughes-Liu  shell  elements  are  derived  from  their  use  of  one-point 
quadrature in the plane of the element.  To suppress the hourglass deformation 
modes  that  accompany  one-point  quadrature,  hourglass  viscous  or  stiffness 
based stresses are added to the physical stresses at the local element level.  The 
discussion of the hourglass control that follows pertains to all one point quadri-
lateral shell and membrane elements in LS-DYNA. 
The hourglass shape vector 𝜏𝐼  is defined as 
𝜏𝐼 = ℎ𝐼 − (ℎ𝐽𝑥̂𝑎𝐽)𝐵𝑎𝐼 
where,  𝑥̂𝑎𝐽  are  the  element  coordinates  in  the  local  system  at  the  Ith  element 
node, 𝐵𝑎𝐼 is the strain displacement matrix, and hourglass basis vector is: 
ℎ =
+1
⎤
⎡
−1
⎥⎥
⎢⎢
+1
−1⎦
⎣
is the basis vector that generates the deformation mode that is neglected by one-
point quadrature.  In the above equations and the remainder of this subsection, 
the Greek subscripts have a range of 2, e.g., 𝑥̂𝑎𝐼 = (𝑥̂1𝐼 , 𝑥̂2𝐼) = (𝑥̂𝐼 , 𝑦̂𝐼). 
The  hourglass  shape  vector then  operates on  the  generalized  displacements  to 
produce the generalized hourglass strain rates 
𝑀 = 𝜏𝐼𝜐̂𝛼𝐼 
𝑞 ̇𝛼
𝐵 = 𝜏𝐼𝜃̂
𝛼𝐼 
𝑞 ̇𝛼
𝑊 = 𝜏𝐼𝜐̂𝑧𝐼 
𝑞 ̇3
where the superscripts M, B, and W denote membrane, bending, and warping 
modes,  respectively.    The  corresponding  hourglass  stress  rates  are  then  given 
by 
𝑄̇𝛼
𝑀 =
QM × 𝐸𝑡𝐴
𝐵𝛽𝐼𝐵𝛽𝐼𝑞 ̇𝛼
𝐵 =
𝑄̇
𝑊 =
QB × 𝐸𝑡3𝐴
192
QW × 𝜅𝐺𝑡3𝐴
12
𝐵 
𝐵𝛽𝐼𝐵𝛽𝐼𝑞 ̇𝛼
𝐵 
𝐵𝛽𝐼𝐵𝛽𝐼𝑞 ̇3
where 𝑡 is the shell thickness.  The hourglass coefficients: QM, QB, and QW are 
generally assigned values between 0.05 and 0.10. 
Finally, the hourglass stresses which are updated using the time step, Δ𝑡, from 
the stress rates in the usual way, that is,  
and the hourglass resultant forces are then 
𝑸𝑛+1 = 𝑸𝑛 + Δ𝑡𝐐̇  
𝑓 ̂
𝐻 = 𝜏𝐼𝑄𝛼
𝑀 
𝛼𝐼
𝐻 = 𝜏𝐼𝑄𝛼
𝐵 
𝑚̂𝛼𝐼
𝑓 ̂
𝑊 
𝐻 = 𝜏𝐼𝑄3
3𝐼
where the superscript H emphasizes that these are internal force contributions 
from the hourglass deformations.  
6. 
IHQ = 7  is  a  linear  total  strain  formulation  of  the  Belytschko-Bindeman  [1993] 
stiffness  form  for  2D  and  3D  solid  elements.    This  linear  form  was  developed 
for visco-elastic material and guarantees that an element will spring back to its 
initial shape regardless of the severity of deformation.   
7.  The default value for QM is 0.1 unless superseded by a nonzero value of QH in 
*CONTROL_HOURGLASS.  A nonzero value of QM supersedes QH. 
8.  Hourglass type 9 is available for hexahedral elements and is based on physical 
stabilization  using  an  enhanced  assumed  strain  method.    In  performance  it  is 
similar  to  the  Belytschko-Bindeman  hourglass  formulation  (type  6)  but  gives 
more  accurate  results  for  distorted  meshes,  e.g.,  for  skewed  elements.    If 
QM = 1.0, it produces accurate coarse bending results for elastic materials.  The 
hourglass  stiffness  is  by  default  based  on  elastic  properties,  hence  the QM  pa-
rameter  should  be  reduced  to  about  0.1  for  plastic  materials  in  order  not  to 
stiffen the structure during plastic deformation.  For materials 3, 18 and 24 there 
is  the  option  to  use  a  negative  value  of  QM.    With  this  option,  the  hourglass 
stiffness  is  based  on  the  current  material  properties,  i.e.,  the  plastic  tangent 
modulus, and scaled by ∣QM∣. 
9.  The default value for IHQ, if not defined on *CONTROL_HOUGRGLASS is as 
follows: 
For shells:  viscous type (1 = 2 = 3) for explicit; stiffness type (4=5) for implicit
For formulation 1 tshells:  type 2. 
10.  For  implicit  analysis,  hourglass  forms  6,  7,  9,  and  10  are  available  for  solid 
elements, and the stiffness form (4 = 5) is available for shells. 
11.  Tshell formulations 2 and 3 have 2 × 2 in-plane integration and therefore do not 
use hourglass control.  
12.  In  the  case  of  tshell  formulation  1,  there  are  two  viscous  hourglass  types 
(IHQ = 1,2) and one stiffness type (IHQ > 2). 
13.  The  hourglass  type  IHQ  has  no  bearing  on  tshell  formulation  5  as  this 
formulation is based on an assumed strain field, similar to formulation 1 solids 
with hourglass type 6.  The hourglass coefficient QM does affect the behavior of 
tshell formulation 5.
Purpose:    The  keyword  *INCLUDE  provides  a  means  of  reading  independent  input 
files containing model data.  The file contents are placed directly at the location of the 
*INCLUDE line. 
*INCLUDE_{OPTION} 
*INCLUDE_AUTO_OFFSET 
*INCLUDE_COMPENSATION_OPTION 
*INCLUDE_MULTISCALE_SPOTWELD 
*INCLUDE_TRIM 
*INCLUDE_UNITCELL
*INCLUDE_{OPTION} 
Available options include: 
<BLANK> 
BINARY 
NASTRAN 
PATH 
PATH_RELATIVE 
STAMPED_SET 
TRANSFORM 
TRANSFORM_BINARY 
STAMPED_PART_{OPTION1}_{OPTION2}_{OPTION3} 
OPTION1: SET 
OPTION2: MATRIX 
OPTION3: INVERSE 
The  BINARY  and  TRANSFORM_BINARY  options  specify  that  the  initial  stress  file, 
dynain, is written in a binary format.  See the keyword *INTERFACE_SPRINGBACK. 
The  PATH  option  defines  a  directory  in  which  to  look  for  the  include  files.    The 
program always searches the local directory first.  If an include file is not found and the 
filename has no path, the program will search for it in all the directories defined by *IN-
CLUDE_PATH.  Multiple paths can defined with one *INCLUDE_PATH definition, i.e., 
*INCLUDE_PATH
Directory_path1
Directory_path2
Directory_path3
Directory  paths  are  read  until  the  next  “*”  card  is  encountered.    A  directory  path  can 
have up to 236 characters . 
The PATH_RELATIVE option is like the PATH option, except all directories are relative 
to  the  location  of  the  input  file.    For  example,  if  “i=/home/test/problems/input.k”  is 
given on the command line, and the input contains
*INCLUDE_PATH_RELATIVE
Includes 
../includes 
then the two directories /home/test/problems/includes and /home/test/includes will be 
searched for include files. 
The STAMPED_PART option applies only to thin shell elements and allows the plastic 
strain and thickness distribution of the stamping simulation to be mapped onto a part in 
the crash model.   
1.  When option 1, SET is used, the PID will be part set ID.  All the parts included 
in this set will be considered in this mapping. 
2.  When  option  2,  MATRIX  is  used,  translation  matrix  will  be  read  directly  and 
the orientation nodes will be ignored. 
3.  When option 3, INVERSE (must be used with MATRIX) is used, the matrix will 
be reversed first. 
When STAMPED_SET is used, the target is a part set ID.  Between the stamped part and 
the crash part, note the following points: 
1.  The outer boundaries of the parts do not need to match since only the regions of 
the crash part which overlap the stamped part are initialized.   
2.  Arbitrary mesh patterns are assumed. 
3.  Element formulations can change. 
4.  Three nodes on each part are used to reorient the stamped part for the mapping 
of the strain and thickness distributions.  After reorientation, the three nodes on 
each part should approximately coincide. 
5.  The number of in plane integrations points can change. 
6.  The number of through thickness integration points can change.  Full interpola-
tion is used. 
7.  The node and element ID's between the stamped part and the crash part do not 
need to be unique. 
The  TRANSFORM  option  allows  for  node,  element,  and  set  ID's  to  be  offset  and  for 
coordinates and constitutive parameters to be transformed and scaled.
Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
FILENAME 
C 
If  the  *INCLUDE  command  is  used  without  options,  multiple  filenames  can  be 
specified, i.e., 
*INCLUDE
Filename1
Filename2
Filename3
which  are  processed  sequentially.    Filenames  are  read  until  the  next  “*”  card  is 
encountered. 
Nastran Card.  Additional Card for the NASTRAN keyword option. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BEAMDF  SHELLDF  SOLIDDF 
Type 
Default 
I 
2 
I 
I 
21 
18 
Stamped Part Card 1.  Additional Card for STAMPED_PART keyword option. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
THICK 
PSTRN 
STRAIN 
STRESS 
INCOUT 
RMAX 
Type 
I 
Default 
none 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
F 
20.0
Stamped Part Card 2a.  Additional card for STAMPED_PART option not ending in_
MATRIX. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
N1S 
N2S 
N3S 
N1C 
N2C 
N3C 
TENSOR 
THKSCL 
Type 
Default 
Remarks 
I 
0 
2 
I 
0 
2 
I 
0 
2 
I 
0 
2 
I 
0 
2 
I 
0 
2 
I 
0 
4 
F 
1.0 
Stamped  Part  (Matrix)  Card  2b.    Additional  card  for  STAMPED_PART_MATRIX 
option. 
5 
6 
7 
8 
  Card 3 
1 
2 
3 
Variable 
R11 
R12 
R13 
Type 
Default 
Remarks 
F 
0 
2 
F 
0 
2 
F 
0 
2 
4 
XP 
F 
0 
2 
Stamped  Part  (Matrix)  Card  3.    Additional  card  for  STAMPED_PART_MATRIX 
option. 
  Card 4 
1 
2 
3 
Variable 
R21 
R22 
R23 
Type 
Default 
Remarks 
F 
0 
2 
LS-DYNA R10.0 
F 
0 
2 
F 
0 
2 
4 
YP 
F 
0 
2 
5 
6
Stamped  Part  (Matrix)  Card  4.    Additional  card  for  STAMPED_PART_MATRIX 
option. 
5 
6 
7 
8 
  Card 5 
1 
2 
3 
Variable 
R31 
R32 
R33 
Type 
Default 
Remarks 
F 
0 
2 
F 
0 
2 
F 
0 
2 
4 
ZP 
F 
0 
2 
Remaining Stamped Part cards are optional.† 
Stamped  Part  Card  6.    Optional  card  for  STAMPED_PART  (with  and  without_MA-
TRIX) keyword option. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ISYM 
IAFTER 
PERCELE
IORTHO 
ISRCOUT 
Type 
I 
I 
F 
I 
I 
Stamped  Part  Card  6.    Optional  card  for  STAMPED_PART  (with  and  without_MA-
TRIX) keyword option. 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
X01 
Y01 
Z01 
Type 
F 
F
Stamped  Part  Card  7.    Optional  card  for  STAMPED_PART  (with  and  without_MA-
TRIX) keyword option. 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
X02 
Y02 
Z02 
X03 
Y03 
Z03 
Type 
F 
F 
F 
F 
F 
F 
Transform Card 1.  Additional card for TRANSFORM keyword option. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IDNOFF 
IDEOFF 
IDPOFF 
IDMOFF 
IDSOFF 
IDFOFF 
IDDOFF 
Type 
I 
I 
I 
I 
I 
I 
I 
Transform Card 2.  Additional card for TRANSFORM keyword option. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IDROFF 
PREFIX 
SUFFIX 
Type 
I 
A 
A 
Transform Card 3.  Additional card for TRANSFORM keyword option. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FCTMAS 
FCTTIM 
FCTLEN 
FCTTEM 
INCOUT1 
Type 
F 
F 
F 
A
Transform Card 4.  Additional card for TRANSFORM keyword option. 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TRANID 
Type 
Default 
I 
0 
  VARIABLE   
FILENAME 
DESCRIPTION
File name of file to be included in this keyword file, 80 characters
maximum.    If  the  STAMPED_PART  option  is  active,  this  is  the 
dynain file containing the results from metal stamping. 
BEAMDF 
LS-DYNA beam element type. Defaults to type 2. 
SHELLDF 
LS-DYNA shell element type.  Defaults to type 21. 
SOLIDDF 
LS-DYNA solid element type.  Defaults to type 18. 
PID 
Part ID of crash part for remapping. 
THICK 
Thickness remap: 
EQ.0: map thickness 
EQ.1: do not map thickness 
EQ.2: average value inside a circle defined by RMAX 
PSTRN 
Plastic strain remap: 
EQ.0: map plastic strain 
EQ.1: do not plastic strain 
EQ.2: average value inside a circle defined by RMAX 
STRAIN 
Strain remap: 
EQ.0: map strains 
EQ.1: do not map strains
VARIABLE   
DESCRIPTION
STRESS 
Stress tensor remap: 
EQ.0:  map stress tensor and history variables 
EQ.1:  do not map stress tensor, only history variables 
EQ.2:  neither map stress tensor nor history variables 
EQ.-1:  map  stress  tensor  in  an  internal  large  format  (binary
files) 
EQ.-3:  do  not  map  stress  tensor  in  an  internal  large  format, 
only history (binary files) 
EQ.1: to save the mapped data to a file called dyna.inc, which
contains  the  mapped  data  for  the  part  that  is  being
mapped.  This option is useful to do mapping using IN-
CLUDE_STAMPED_PART  and  then  save  the  mapped 
data for future use.  When INCOUT is set to 2, the output 
file is in dynain format and the file name is dynain_xx (xx 
is the part or part set id); and when INCOUT is set to 3,
the output file is in NASTRAN format, and the file name
is: nastran_xx. 
EQ.2: to save the mapped data for the specified part (PID) to a
file called dynain_PID. 
EQ.3: to save the mapped data for the specified part (PID) to a
file called nastran_PID (in nastran format) 
Search radius.  LS-DYNA remaps history variables from the mesh
of  the  stamped  part  to  the  mesh  of  the  crash  part  with  a  spatial
tolerance  of  RMAX.    If  an  element  in  the  crash  part  lies  within
RMAX of the stamped part, data will be mapped to that element.
If  set  less  than  0.001,  RMAX  automatically  assumes  the  default
value of 20. 
First of 3 nodes needed to reorient the stamped part. 
Second of 3 nodes needed to reorient the stamped part. 
Third of 3 nodes needed to reorient the stamped part. 
First of 3 nodes needed to reorient the crash model part. 
Second of 3 nodes needed to reorient the crash model part. 
Third of 3 nodes needed to reorient the crash model part. 
INCOUT 
RMAX 
N1S 
N2S 
N3S 
N1C 
N2C 
N3C
VARIABLE   
DESCRIPTION
TENSOR 
Tensor remap: 
EQ.0: map tensor data from history variables.   
EQ.1: do not map tensor data from history variables 
THKSCL 
Thickness scale factor. 
R11, R12, R33 
Components of the transformation matrix. 
XP, YP, ZP 
Translational distance. 
ISYM 
Symmetric switch 
EQ.0: no symmetric mapping 
EQ.1: 𝑦𝑧 plane symmetric mapping 
EQ.2: 𝑧𝑥 plane symmetric mapping 
EQ.3: 𝑧𝑥 and 𝑦𝑧 planes symmetric mapping 
EQ.4: user defined symmetric plane mapping 
IAFTER 
Mirroring sequence switch 
EQ.0: generate a symmetric part before transformation 
EQ.1: generate a symmetric part after transformation 
PERCELE 
Percentage  of  elements  that  should  be  mapped  to  proceed
(default = 0); otherwise an error termination occurs.  See Remark 
6. 
IORTHO 
Location  of  the  material  direction  cosine  in  the  array  of  history
variables of an orthotropic material.  See Remark 5. 
ISRCOUT 
Optional output of stamped part after transformation(s) 
EQ.0: no output is written 
NE.0: keyword output file “srcmsh_<ISRCOUT>” is created 
X01, Y01, Z01 
First point in the symmetric plane (required if ISYM.NE.0) 
X02, Y02, Z02 
Second point in the symmetric plane 
X03, Y03, Z03 
Third point in the symmetric plane 
IDNOFF 
Offset to node ID.
VARIABLE   
DESCRIPTION
IDEOFF 
Offset to element ID. 
IDPOFF 
Offset  to  part  ID,  nodal  rigid  body  ID,  constrained  nodal  set  ID,
Rigidwall ID, and *DATABASE_CROSS_SECTION. 
IDMOFF 
Offset to material ID and equation of state ID. 
IDSOFF 
Offset to set ID. 
IDFOFF 
Offset to function ID, table ID, and curve ID. 
IDDOFF 
to  any 
Offset 
FUNCTION, TABLE, and CURVE options . 
through  *DEFINE  except 
ID  defined 
the
IDROFF 
Used for all offsets except for those listed above. 
PREFIX 
SUFFIX 
FCTMAS 
FCTTIM 
Prefix  added  to  the  beginning  of  the  titles/heads  defined  in  the
keywords 
for
examples) of the included file.  A dot, “.”, is automatically added
between the prefix and the existing title.  
(like  *MAT,  *PART,  *SECTION,  *DEFINE, 
Suffix  added  to  the  end  of  the  titles/heads  defined  in  the 
keywords of the included file.  A dot, “.”, is automatically added
between the suffix and the existing title. 
Mass  transformation  factor. 
When the original mass units are in tons and the new unit is kg. 
  For  example,  FCTMAS = 1000. 
Time transformation factor.  For example, FCTTIM=.001 when the
original  time  units  are  in  milliseconds  and  the  new  time  unit  is
seconds. 
FCTLEN 
Length transformation factor. 
FCTTEM 
INCOUT1 
Temperature  transformation  factor  consisting  of  a  four  character 
flag:  FtoC  (Fahrenheit  to  Centigrade),  CtoF,  FtoK,  KtoF,  KtoC,
and CtoK. 
Set  to  1  for  the  creation  of  a  file,  DYNA.INC,  which  contains  the 
transformed  data.    The  data  in  this  file  can  be  used  in  future
include files and should be checked to ensure that all the data was
transformed correctly. 
TRANID 
Transformation ID, if 0 no transformation will be applied. 
See the input DEFINE_TRANSFORMATION.
*INCLUDE_{OPTION} 
1.  Scalability.    To  make  the  input  file  easy  to  maintain,  this  keyword  allows  the 
input  file  to  be  split  into  subfiles.    Each  subfile  can  again  be  split  into  sub-
subfiles  and  so  on.    This  option  is  beneficial  when  the  input  data deck  is  very 
large.  Consider the following example: 
*TITLE 
full car model 
*INCLUDE 
carfront.k 
*INCLUDE 
carback.k 
*INCLUDE 
occupantcompartment.k 
*INCLUDE 
dummy.k 
*INCLUDE 
bag.k 
*CONTACT 
⋮  
*END 
Note that the command *END terminates the include file. 
The  carfront.k  file  can  again  be  subdivided  into  rightrail.k,  leftrail.k,  battery.k, 
wheel-house.k,  shotgun.k,  etc..    Each  *.k  file  can  include  nodes,  elements, 
boundary conditions, initial conditions, and so on. 
*INCLUDE 
rightrail.k 
*INCLUDE 
leftrail.k 
*INCLUDE 
battery.k 
*INCLUDE 
wheelhouse.k  
*INCLUDE 
shotgun.k 
⋮  
*END 
2.  Reorienting  the  Result  of  a  Stamping  Simulation  for  STAMPED_PART 
option.  When defining *INCLUDE_STAMPED_PART the target mesh must be 
read in before the include stamped part. 
N1S,  N2S,  N3S,  N1C,  N2C,  and  N3C  are  used  for  transforming  the  stamped 
part to the crash part, such that it is in the same position as the crash part.  If the 
stamped part is in the same position as the crash part then N1S, N2S, N3S, N1C,
N2C, N3C can all be set to 0.  Note:  If these 6 nodes are input as 0, LS-DYNA 
will not transform the stamped part. 
When  symmetric  mapping  is  used  (ISYM  is  not  zero),  the  three  points  should 
not be in one line. 
If ISYM = 0, 1, 2, or 3, only the first point (X01,Y01, Z01) is needed 
If ISYM = 4, all the three points are needed 
3.  Path  Length  Limitations.    Filenames  and  pathnames  are  limited  to  236 
characters  spread  over  up  to  three  80  character  lines.    When  2  or  3  lines  are 
needed  to  specify  the  filename  or  pathname,  end  the  preceding  line  with  "˽+" 
(space followed by a plus sign) to signal that a continuation line follows.  Note 
that the "˽+" combination is, itself, part of the 80 character line; hence the maxi-
mum number of allowed characters is 78 + 78 + 80 = 236. 
4.  Mapping  Material  Data  for  Springback  for  STAMPED_PART  option.  
Certain  material  models  (notably  Material  190)  have  tensor  data  stored  within 
the history variables.   Within material subroutines this data is typically stored 
in element local coordinate systems.  In order to properly map this information 
between  models  it  is  necessary  to  have  the  tensor  data  present  on  the  *INI-
TIAL_STRESS_SHELL  card  and  have  it  stored  in  global  coordinates.    During 
mapping the data is then converted into the local coordinate system of the crash 
mesh.  This data can be dumped into the dynain file that is created at termina-
tion  time  if  the  parameter  FTENSR  is  set  to  0  on  the  *INTERFACE_SPRING-
BACK_DYNA3D  card.    Currently,  the  only  material  model  that  supports 
mapping of element history tensor data is Material 190. 
5. 
IORTHO.  If IORTHO is set, correct mapping between non-matching meshes is 
invoked for the directions of orthotropic materials.  A list of appropriate values 
for several materials is given here: 
IORTHO.EQ.1:  materials 23, 122, 157, 234 
IORTHO.EQ.3:  materials 22, 33, 36, 133, 189, 233, 243 
IORTHO.EQ.4:  material 59 
IORTHO.EQ.6:  materials 58, 104, 158 
IORTHO.EQ.8:  materials 54, 55 
IORTHO.EQ.9:  material 39 
IORTHO.EQ.10:  material 82
IORTHO.EQ.13:  materials 2, 86, 103 
6.  Mapping  Mismatch  with  STAMPED_PART  option.    Sometimes  during 
mapping the two  meshes (stamp  mesh and  crash mesh) do not fit exactly and 
therefore  not  all  elements  of  the  new  mesh  get  results  from the  old  mesh.    In-
formation  about  the  total  number  of  crash  elements  which  are  /  are  not 
mapped is given in the message file.  By default (PERCELE=0), the calculation 
continues even with zero number of mapped elements.  With PERCELE>0 the 
percentage of minimum number of elements can be defined, which have to be 
mapped.  If a percentage less than PERCELE is mapped, calculation stops with 
an error termination. 
7.  NASTRAN Option.  The transformed LS-Dyna deck for *INCLUDE_NASTRAN 
will be automatically written to file DYNA.INC.
*INCLUDE 
Purpose:    This  particular  *INCLUDE  keyword  offsets  node  and  element  IDs  to  avoid 
duplication during stamping simulations.  In stamping simulations the rigid tools often 
undergo  several  iterations  of  modifications.    The  node  or  element  IDs  comprising  the 
new tools sometimes conflict with other parts of the model, which makes it difficult to 
automate  the  process  simulation.    This  keyword  automatically  checks  for  and  fixes 
duplicate IDs.  The *CONTROL_FORMING_MAXID keyword is related. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
FILENAME 
C 
  VARIABLE   
DESCRIPTION
FILENAME 
File name to be included. 
Remarks: 
This  keyword  can  be  used  to  offset  element  and  node  IDs  of  the  tooling.    The  keyword 
will  not  offset  meshes  with  initial  stress  and  strain  information.    As  such,  sheet  blank 
(including dynain file) should always  be included first using the *INCLUDE keyword, 
followed by *INCLUDE_AUTO_OFFSET to offset tooling mesh IDs which do not have 
stress and strain information. 
Incoming  element  and  node  IDs  of  the  tooling  mesh  files  such  as  the  punch,  die,  and 
binder, can be overlapped with each other, or overlapped with those on the sheet blank.  
Multiple  *INCLUDE_AUTO_OFFSET  can  be  used  to  include  punch,  die,  binder 
separately, if desired.  For example, four different components of the tooling, upper die, 
lower  punch,  binder  and  gage  pins  can  be  included  and  their  element  and  node  IDs 
properly offset after those of a gravity-loaded sheet blank: 
*INCLUDE 
gravity.dynain 
*INCLUDE_AUTO_OFFSET 
upperdie.k 
*INCLUDE_AUTO_OFFSET 
lowerpunch.k 
*INCLUDE_AUTO_OFFSET 
binder.k 
*INCLUDE_AUTO_OFFSET 
pins.k 
All of the included meshes can have conflicting mesh IDs starting from “1”.  Mesh IDs 
will  be  offset  and  reordered  in  the  order  of  the  tool  inclusion  using  *INCLUDE_AU-
TO_OFFSET.    Included  tool  files  whose  mesh  IDs  do  not  overlap with  those  on  either 
the  blank  or  other  tools  will  not  be  offset  or  reordered.    In  many  circumstances  this 
feature allows the user to bypass the metal forming GUI when updating just one or two 
tooling pieces. 
Revision information: 
This  feature  is  available  in  SMP  and  MPP  starting  in  LS-DYNA  Revision  92417.  
Revision  117818  extends  the  keyword  to  beams  (used  to  model  draw  beads,  for 
example) and solids.
*INCLUDE_COMPENSATION_{OPTION} 
Purpose:    This  group  of  keywords  allow  for  the  inclusion  of  stamping  die  geometry 
information  for  springback  compensation.    In  addition,  trim  curves  from  the  target 
geometry  can  be  included  for  mapping  onto  the  intermediate  compensated  tool 
geometry,  which  can  be  used  for  the  next  compensation  iteration.    Furthermore, 
compensation  can  be  done  for  a  localized  tool  region.    These  keywords  must  be  used 
together with *INTERFACE_COMPENSATION_NEW. 
Options available include: 
BLANK_BEFORE_SPRINGBACK 
BLANK_AFTER_SPRINGBACK 
DESIRED_BLANK_SHAPE 
COMPENSATED_SHAPE 
CURRENT_TOOLS 
TRIM_CURVE 
CURVE 
ORIGINAL_DYNAIN 
SPRINGBACK_INPUT 
COMPENSATED_SHAPE_NEXT_STEP 
SYMMETRIC_LINES 
ORIGINAL_RIGID_TOOL 
NEW_RIGID_TOOL 
ORIGINAL_TOOL 
UPDATED_BLANK_SHAPE 
UPDATED_RIGID_TOOL
Blank  Before  Springback  Card.    Additional  card  for  BLANK_BEFORE_SPRING-
BACK keyword option. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME 
C 
blank0.tmp 
Blank  After  Springback  Card.    Additional  card  for  BLANK_AFTER_SPRINGBACK 
keyword option. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME 
C 
spbk.tmp 
Desired Blank Shape Card.  Additional card for DESIRED_BLANK_SHAPE keyword 
option. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME 
C 
reference0.dat
Compensated  Shape  Card.    Additional  card  for  COMPENSATED_SHAPE  keyword 
option. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME 
C 
reference1.dat 
Current Tools Card.  Additional card for CURRENT_TOOLS keyword option. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME 
C 
rigid.tmp 
Generic  Filename  Card.    Additional  Card  for  TRIM_CURVE,  CURVE,  ORIGINAL_-
DYNAIN,  SPRINGBACK_INPUT,  COMPENSATED_SHAPE_NEXT_STEP,  ORIGI-
NAL_RIGID_TOOL,  NEW_RIGID_TOOL,  ORIGINAL_TOOL,  UPDATED_BLANK_-
SHAPE, and UPDATED_RIGID_TOOL keyword options. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME 
C 
See Remarks
Symmetric Lines Cards.  Additional card for SYMMETRIC_LINES keyword option. 
  Card 1 
1 
2 
Variable 
SYMID 
SYMXY 
5 
6 
7 
8 
3 
X0 
F 
4 
Y0 
F 
I 
Type 
Default 
I 
1 
  VARIABLE   
FILENAME 
none 
0.0 
0.0 
DESCRIPTION
For  options  below,  input  the  name  of  the  keyword  files
containing  nodes  and  elements  information,  with  adaptive
constraints if exist.  Currently all sheet blanks must have the same
numbers of nodes and elements. 
BLANK_BEFORE_SPRINGBACK, 
BLANK_AFTER_SPRINGBACK, 
DESIRED_BLANK_SHAPE, 
COMPENSATED_SHAPE, 
CURRENT_TOOLS, 
COMPENSATED_SHAPE_NEXT_STEP 
For  option  ORIGINAL_DYNAIN,  input  the  dynain  file  name 
from  LS-DYNA  simulation  (for  example,  trimmed  panel  from
ITER0  baseline  simulation)  which  contains  model  information, 
adaptive  constraints,  stress  and  strain  tensor  information.    This
keyword  is  to  be  used  in  conjunction  with  *INTERFACE_COM-
PENSATION_NEW_ACCELATOR. 
the  file  name  of 
For  option  SPRINGBACK_INPUT,  give 
springback  simulation 
input  deck  for  the  baseline  ITER0 
simulation.  This keyword is to be used in conjunction with *IN-
TERFACE_COMPENSATION_NEW_ACCELATOR. 
For  option  TRIM_CURVE,  input  the  name  of  the  keyword  file
containing  𝑥,  𝑦,  𝑧  coordinates  as  defined  using  keyword  *DE-
FINE_CURVE_TRIM_3D  (only  TCTYPE = 0,  or  1  is  supported). 
This  option  is  used  to  map  the  trim  curve  to  the  new,
VARIABLE   
DESCRIPTION
compensated tooling mesh for next iterative simulation. 
For option CURVE, input the name of the keyword file containing
𝑥, 𝑦, 𝑧 coordinates of two curves defining the compensation zone,
using  keywords:  *DEFINE_CURVE_COMPENSATION_CON-
STRAINT_BEGIN,  and,  *DEFINE_CURVE_COMPENSATION_-
CONSTRAINT_END. 
  This  option  is  for  compensation  of
localized tooling areas. 
All  foregoing  keyword  options  are  used  together  with  *INTER-
FACE_COMPENSATION_NEW. 
For  options  ORIGINAL_RIGID_TOOL  and  NEW_RIGID_TOOL, 
input the file names of the keyword file containing meshes of the
rigid  tools.    This  option  is  used  to  smooth  distorted  meshes  of 
localized tool surfaces.  These keyword options are used together
with 
*INTERFACE_COMPENSATION_NEW_LOCAL_-
SMOOTH. 
For option ORIGINAL_TOOL, input the file name of the original 
tool  (without  any  compensation)  mesh  containing  nodes  and 
elements  information  in  keyword  format.    This  option  allow  the
use  of  the  original  tool  mesh,  which  is  of  higher  quality,  in  the
iterative  compensation  runs,  to  minimize  the  tool  surface  mesh
distortion in the addendum and binder areas of the compensated 
tool  .    These  keyword  options  are  used  together
with *INTERFACE_COMPENSATION_NEW. 
For  options  UPDATED_BLANK_SHAPE,  and  UPDATED_-
RIGID_TOOL, input the respective mesh information in keyword
format.    The  updated  blank  shape  is  the  blank  formed  (or 
trimmed)  shape  based  on  the  new  tool  (die)  geometry.    These
options  allow  for  updating  of  compensated  tool  shape  for  small
part shape changes, without the need to go through a full-blown 
iterative compensation loop again .  The options are 
used  together  with  *INTERFACE_COMPENSATION_NEW_-
PART_CHANGE, among others. 
SYMID 
ID of the symmetric condition being defined.
VARIABLE   
DESCRIPTION
SYMXY 
Code defining symmetric boundary conditions: 
EQ.1: symmetric about 𝑦-axis. 
EQ.2: symmetric about 𝑥-axis. 
X0, Y0 
Coordinates of a point on the symmetric plane. 
Default Filenames: 
Keyword Option 
Default Filename 
UPDATED_BLANK_SHAPE 
updatedpart.tmp 
UPDATED_RIGID_TOOL 
newrigid.tmp 
About various options: 
This group of keywords is used in conjunction with *INTERFACE_COMPENSATION_-
NEW,  to  compensate  stamping  tool  shapes  for  springback  with  an  iterative  method.  
The method approaches the final target design intent from two opposite directions from 
iteration to iteration.  A typical successful compensation requires about 3 to 4 iterations. 
1.  BLANK_BEFORE_SPRINGBACK. 
  When  the  option  BLANK_BEFORE_-
SPRINGBACK  is  used,  the  included  file  is  the  mesh  information  in  keyword 
format  in  the  first  state  (from  d3plot)  of  the  springback  simulation,  or  the 
“dynain” file after trimming (before springback and with no mesh coarsening).  
The default file name is “blank0.tmp”. 
2.  BLANK_AFTER_SPRINBACK.    When  the  option  BLANK_AFTER_SPRIN-
BACK is used, the included file is the “dynain” file after springback, or the last 
state  mesh  (from  d3plot)  of  the  springback.    The  default  file  name  is 
“spbk.tmp”. 
3.  DESIRED_BLANK_SHAPE.    When  the  option  DESIRED_BLANK_SHAPE  is 
used,  the  included  file  is  the  “dynain”  file  after  trimming  in  the  first  iteration.  
This file never changes in all subsequent iterative compensation.  The file name 
default is “reference0.dat”. 
4.  COMPENSATED_SHAPE.  When the option COMPENSATED_SHAPE is used, 
the included file for the first iteration, is a “dynain” file, same as in the option 
DESIRED_BLANK_SHAPE; and for the following compensation iterations, this
file is obtained from the file “disp.tmp” generated as an output file during the 
previous compensation iteration.  The default file name is “reference1.dat”. 
5.  CURRENT_TOOLS.  When the option CURRENT_TOOLS is used, the included 
file is the file containing the tool mesh in the keyword format.  This is the tool 
mesh from the last compensation run and used for the current forming simula-
tion.  The draw bead nodes have to be included in this file so that they will be 
modified together with the rigid tools.  The default file name is “rigid.tmp”, and 
if  the  file  is  named  as  “rigid0.tmp”  the  elements  of  the  tools  get  refined  along 
the outline of the part. 
6.  TRIM_CURVE.    When  the  option  TRIM_CURVE  is  used,  trim  curves  off  the 
current  tools  are  mapped  onto  the  compensated  tools  for  the  trimming  opera-
tion in the next iteration. 
If the trimming simulation uses the IGES format trim curves, a new file “geo-
cur.trm” will be generated at the end of the trimming simulation.  The file basi-
cally  contains  XYZ  data  of  the  trim  curves  in  keyword  *DEFINE_CURVE_-
TRIM_{OPTIONS},  which  is  used  for  the  compensation  run.    Note  that  the 
variable TCTYPE in the keyword must be set to “0” (or “1”) for the compensa-
tion.    Length  of  lines  everywhere  in  the  compensated  part  are  calculated  ac-
cording  to  springback  amounts  (including  the  die  expansion  factors,  therefore 
no die expansion needs to be included in the NC machining of the compensated 
tooling).    These  mapped  trim  curves  can  be  used  for  die  development  on  the 
compensated tools and for laser trimming of stamped panels.  Procedures out-
line  in  keyword  manual  pages  *INTERFACE_BLANKSIZE  can  be  followed  to 
convert in LS-PrePost IGES file of the trim curves to XYZ format (and vice ver-
sa) used in this keyword. 
In  an  example  keyword  input  shown  below,  the  file  name  for  this  option  is 
trimcurves.k.  The format is in XYZ format, written with LS-PrePost: 
*DEFINE_CURVE_TRIM_3D 
$#    tcid    tctype      tflg      tdir     tctol      toln     nseed 
      1116         1         1               0.100         1 
$#                cx                  cy                  cz 
           178.05170          -326.24771           51.924496 
           177.77397          -301.90869           50.288792 
           177.29764          -265.39716           48.594341 
... 
7.  CURVE.  When the option CURVE is used, it allows for die face compensation 
of a local region in a stamping die.  This option is used in conjunction with two 
more keywords defining two enclosed curves that form the compensation zone 
in  position  coordinates  𝑥,  𝑦,  𝑧:  *DEFINE_CURVE_COMPENSATION_CON-
STRAINT_BEGIN, 
*DEFINE_CURVE_COMPENSATION_CON-
STRAINT_END.    Detailed  usage  of  these  two  keywords  is  available  in  the 
related manual pages. 
and
*INCLUDE_COMPENSATION 
The  following  example  is  for  compensation  of  a  localized  area,  defined  by  the  file 
curves.k.    Trim  lines  are  mapped  onto  the  new  compensated  rigid  tool,  with 
trimcurves.k.    Both  files  which  were  generated  by  LS-PrePost  4.0  are  in  the  “XYZ 
format”.  A detailed explanation of each keyword is given in the manual pages related 
to *INTERFACE_COMPENSATION_NEW. 
*KEYWORD 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- 
*INTERFACE_COMPENSATION_NEW 
$   METHOD        SL        SF     ELREF      PSID    UNDRCT    ANGLE NLINEAR 
         8    10.000     1.000         0         1         0      0.0       1 
*INCLUDE_COMPENSATION_BLANK_BEFORE_SPRINGBACK 
blank0.k 
*INCLUDE_COMPENSATION_BLANK_AFTER_SPRINGBACK 
spbk.k 
*INCLUDE_COMPENSATION_DESIRED_BLANK_SHAPE 
reference0.k 
*INCLUDE_COMPENSATION_COMPENSATED_SHAPE 
reference1.k 
*INCLUDE_COMPENSATION_CURRENT_TOOLS 
tools.k 
*INCLUDE_COMPENSATION_TRIM_CURVE 
trimcurves.k 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ For compensation of a localize region only, add the following keyword: 
*INCLUDE_COMPENSATION_CURVE 
curves.k 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
*SET_PART_LIST 
$      PSID 
         1 
$      PID 
         3 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- 
*END 
The  option  ORIGINAL_DYNAIN  and  SPRINGBACK_INPUT  are  used  together  with 
keyword  *INTERFACE_COMPENSATION_NEW_ACCELATOR,  for  a  springback 
compensation  with  a  faster  convergence  rate  and  a  simplified  user  interface.    For 
detailed  usage,  please  refer  to  manual  pages  under  *INTERFACE_COMPEN-
STION_{OPTION}.  Here a complete keyword input is provided: 
*KEYWORD 
*INTERFACE_COMPENSATION_NEW_ACCELATOR 
$   ISTEPS      TOLX      TOLY      TOLZ    OPTION 
         3      0.20      0.20       0.2        1 
*INCLUDE_COMPENSATION_ORIGINAL_DYNAIN 
./case20trimmed.dynain 
*INCLUDE_COMPENSATION_SPRINGBACK_INPUT 
./spbk.dyn 
*END 
The  option  COMPENSATED_SHAPE_NEXT_STEP  enables  compensation  of  tools  for 
the next die process.  It is used in conjunction with keyword *INTERFACE_COMPEN-
SATION_NEW_MULTI_STEPS, which is discussed in the corresponding manual pages.  
Here a complete input deck is given below:
*KEYWORD 
*INTERFACE_COMPENSATION_NEW_MULTI_STEPS 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
$   METHOD        SL        SF     ELREF      PSID    UNDRCT     ANGLE   NLINEAR 
         8     6.000      1.00         1         1         0         0         1 
*INCLUDE_COMPENSATION_DESIRED_BLANK_SHAPE 
reference0.tmp 
*INCLUDE_COMPENSATION_COMPENSATED_SHAPE_NEXT_STEP 
Reference1_flanging.tmp 
*INCLUDE_COMPENSATION_CURRENT_TOOLS 
rigid.tmp 
*SET_PART_LIST 
$      PSID 
          1 
$       PID 
          2 
*END 
The option SYMMTRIC_LINES applies to compensation Method 7 and 8, as discussed 
in  *INTERFACE_COMPENSATION_NEW.    In  a  complete  keyword  input  example 
below, part set ID 1 is being compensated with symmetric boundary condition about X-
axis.  The symmetric plane passes a point with coordinates of x = 101.5, and y = 0.0.  
*KEYWORD 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
$*INTERFACE_COMPENSATION_NEW 
$ Method = 8 changes the binder; Method = 7 binder/P.O.  no changes. 
*INTERFACE_COMPENSATION_NEW 
$   METHOD        SL        SF     ELREF      PSID    UNDRCT     ANGLE   NLINEAR 
         7    10.000     1.000         2         1         1       0.0         1 
*INCLUDE_COMPENSATION_BLANK_BEFORE_SPRINGBACK 
./state1.k 
*INCLUDE_COMPENSATION_BLANK_AFTER_SPRINGBACK 
./state2.k 
*INCLUDE_COMPENSATION_DESIRED_BLANK_SHAPE 
./state1.k 
*INCLUDE_COMPENSATION_COMPENSATED_SHAPE 
./state1.k 
*INCLUDE_COMPENSATION_CURRENT_TOOLS 
./currenttools.k 
*INCLUDE_COMPENSATION_SYMMETRIC_LINES 
$    SYMID     SYMXY        X0        Y0 
         1         2     101.5       0.0 
$ SYMXY = 2: symmetric about X-axis 
*SET_PART_LIST 
$      PSID 
         1 
$      PID 
         1 
*END 
The options ORIGINAL_RIGID_TOOL and NEW_RIGID_TOOL are used together with 
*INTERFACE_COMPENSATION_NEW_LOCAL_SMOOTH,  and  *SET_NODE_LIST_-
SMOOTH, to smooth local areas of distorted meshes of a tooling surface.  Details can be 
found 
*INTERFACE_COMPENSATION_NEW_LOCAL_-
SMOOTH. 
in  manual  pages 
for 
The  option  ORIGINAL_TOOL  is  used  to  obtain  a  smoother  mesh  for  the  addendum 
and binder region for the current compensation, using the original tool mesh (of better
quality) instead of the last compensated tool mesh (maybe distorted).  This reduces the 
accumulative error in mesh extrapolation outside of the trim lines.  Details can be found 
in manual pages for *INTERFACE_COMPENSATION_NEW. 
The  options  UPDATED_BLANK_SHAPE,  and  UPDATED_RIGID_TOOL  calculate  a 
new  compensated  tool  shape  according  to  the  updated  blank  shape,  thus  eliminating 
the need to go through a full-blown iterative compensation loop again.  Note that these 
options  are  intended  only  for  small  part  changes  that  do  not  substantially  affect  the 
amount of springback.  More details can be found in manual pages for *INTERFACE_-
COMPENSATION_NEW_PART_CHANGE.  
Revision information: 
The option TRIM_CURVE is available starting in Revision 60398.   The options ORIGI-
NAL_DYNAIN,  and  SPRINGBACK_INPUT  are  available  starting  in  Revision  61264.  
The  option  COMPENSATED_SHAPE_NEXT_STEP  is  available  starting  in  Revision 
61406.    The  option  CURVE  is  available  starting  in  Revision  62038.    The  option  SYM-
METRIC_LINES  is  available  starting  in  Revision  63618  (updated  in  Rev.    83711).    The 
options of ORIGINAL_RIGID_TOOL and NEW_RIGID_TOOL are available starting in 
Revision  73850.    The  option  ORIGINAL_TOOL  is  available  starting  in  Revision  82701.  
The  options  UPDATED_BLANK_SHAPE,  and  UPDATED_RIGID_TOOL  are  available 
starting in Revision 82698. 
.
*INCLUDE_MULTISCALE_SPOTWELD 
Purpose:  To define a type of MULTISCALE spot weld to be used for coupling and for 
modeling of spot weld failure. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TYPE 
Type 
I 
Default 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
  VARIABLE   
TYPE 
FILENAME 
C 
none 
DESCRIPTION 
TYPE  for  this  multiscale  spot  weld.    This  type  is  used  in  the
keyword  *DEFINE_SPOTWELD_MULTISCALE. 
  Any  unique
integer will do. 
FILENAME 
Name of file from which to read the spot weld definition. 
Remarks: 
This capability is available only in the MPP version of LS-DYNA. 
With  the  multiscale  spot  weld  feature  heuristic  spot  weld  models  are  replaced  with 
zoomed-in  geometrically  and  constitutively  correct  continuum  models,  which,  in  turn 
are  coupled  to  the  large-scale  calculation  without  reducing  the  time  step.    In  some 
respects, multiscale models are similar to the “hex spot weld assemblies,” capability but 
more  general  in  terms  of  their  geometry.    Because  the  spot  weld  models  are  run  in  a 
separate process, they can run at a much  smaller time step without slowing down the 
rest of the simulation.  A brief outline of their use looks like this:
•  The user creates one (or more) detailed models of their spot welds, and includes 
these  definitions  into  their  model  using  the  keyword  *INCLUDE_MULTI-
SCALE_SPOTWELD 
•  The user indicates which beam (or hex assembly) spot welds should be coupled 
to these models via the keyword *DEFINE_SPOTWELD_MULTISCALE 
•  When MPP-DYNA is started, a special (MPI dependent) invocation is required in 
order to run in a “multiple program” mode.  Effectively, two separate instances 
of  MPP-DYNA  are  started  together,  one  to  run  the  full  model  and  a  separate 
instance to run the spot welds. 
•  As  the  master  process  runs,  each  cycle  it  communicates  to  the  slave  process 
deformation information for the area surrounding each coupled spot weld.  The 
slave  process  imposes  this  deformation  on  the  detailed  spot  welds,  computes  a 
failure flag for each, and communicates this back to the master process. 
•  The  coupled  spot  welds  in  the  master  process  have  their  failure  determined 
solely by these failure flags. 
The file referred to on the *INCLUDE_MULTISCALE_SPOTWELD card should contain 
one generic instance of a detailed  spot weld.  For each coupled spot weld in the  main 
model,  a  specific  instance  of  this  spot  weld  will  be  generated  which  is  translated, 
rotated,  and  scaled  to  match  the  spot  weld  to  which  it  is  coupled.    In  this  way,  many 
spot welds can be coupled with only a single *INCLUDE_MULTISCALE_SPOTWELD.  
The  included  file  should  contain  everything  required  to  define  the  spot  weld,  such  as 
*MAT and *PART definitions, any required *DEFINE_CURVEs, etc., as well as *NODE 
and *ELEMENT definitions.  In order for the translation and scaling to work properly 
there are some assumptions made about the spot weld model: 
•  It consists entirely of solid elements. 
•  The 𝑧-axis is aligned with the coupled spot weld in the main model, with 𝑧 = 0 
and 𝑧 = 1 at the two ends of the spot weld. 
•  The cross sectional area of the spot weld in the 𝑥𝑦 plane is equal to 1. 
•  That  portion  of  the  “top”  and  “bottom”  of  the  spot  weld  that  are  coupled  are 
identified using a single *SET_NODE_LIST card. 
•  One  *BOUNDARY_COUPLED  card  referencing  the  *SET_NODE_LIST  of  the 
boundary nodes is required.  It must specify a coupling type of 2 and a coupling 
program of 1. 
•  The spot weld model does not support *INCLUDE cards. 
Failure  of  the  fine  model  is  determined  topologically.    Any  element  of  the  spot  weld 
having  all  four  nodes  of  one  of  its  faces  belonging  to  the  *SET_NODE_LIST  of  tied 
nodes  is  classified  as  a  “tied”  element.    The  “tied”  elements  are  partitioned  into  two 
disjoint  sets:  the  “top,”  and  “bottom”.    When  there  is  no  longer  a complete  path  from 
any “top” to any “bottom” element (where a “path” passes through non-failed elements
that  share  a  common  face),  then  the  spot  weld  has  failed.    Note  that  this  places  some 
restrictions  on  the  *SET_NODE_LIST  and  element  geometry,  namely  that  some  “tied” 
elements exist, and the set of “tied” elements consists of exactly two disjoint subsets. 
The  specifics  of  launching  a  multi-program  MPI  program  are  installation  dependent.  
But  the  idea  behind  running  a  coupled  model  is  that  you  want  to  run  one  set  of  MPI 
ranks as if you were running a normal MPP-DYNA job, such as: 
mpirun –np 4 mppdyna i=input.k memory=200m p=pfile 
and a second set with just the command line argument “slave” (no input file): 
mpirun –np 4 mppdyna slave memory=100m p=pfile 
The  main  instance  knows  to  look  for  the  slave  (because  of  the  presence  of  the  *IN-
CLUDE_MULTISCALE_SPOTWELD card), and will run the main model.  The “slave” 
instance will run all the detailed spot weld models.  Due to the nature of the coupling, 
the main model cannot progress when the detailed spot welds are being processed, nor 
can  the  detailed  spot  welds  run  while  the  main  model  is  being  computed.    From  a 
processor efficiency standpoint, it therefore makes sense to run as many slave processes 
as master processes, and run them on the same CPUs, so that each processing core has 
one slave and one master process running on it.   But you don’t have to – the processes 
are independent and you can have any number of either.
*INCLUDE_TRIM 
Purpose:  This keyword is developed to reduce memory requirements and CPU time (as 
compared with *INCLUDE) during trimming in sheet metal forming.  This keyword is 
intended  to  be  used  together  with  the  *DEFINE_CURVE_TRIM_OPTION  and  *ELE-
MENT_TRIM keywords. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
FILENAME 
C 
  VARIABLE   
DESCRIPTION
FILENAME 
File name of the part to be trimmed. 
General remarks: 
The name of the file to be trimmed should be included in a usual LS-DYNA input file 
for trimming, as is in *INCLUDE.  Model information, stress and strain tensors should 
be  all  in  one  dynain  file  generated  from  LS-DYNA  simulation.    For  example,  a  drawn 
panel from a previous simulation can be included in a current trim input file as follows, 
*INCLUDE_TRIM 
Drawnpanel.dynain 
*ELEMENT_TRIM 
⋮ 
*DEFINE_CURVE_TRIM_3D 
⋮ 
*CONTROL_ADAPTIVE_CURVE 
⋮ 
This  feature  has  been  developed  in  conjunction  with  the  Ford  Motor  Company  Research 
and Advanced Engineering Laboratory, and is implemented in LS-PrePost as of version 4.0 
under the metal forming application under eZ-Setup (http://ftp.lstc.com/anonymous/
outgoing/lsprepost/4.0/metalforming/).    Compared  with  *INCLUDE,  this  keyword 
draws much less computer memory and runs much faster. 
Furthermore,  in  case  where  to-be-trimmed  sheet  blank  has  no  stress  and  strain 
information  (no  *INITIAL_STRESS_SHELL,  and  *INITIAL_STRAIN_SHELL  cards 
present in the sheet blank keyword/dynain file), the bare *INCLUDE keyword must be 
used.
*INCLUDE 
Referring to the table below (parts courtesy of the Ford Motor Company), compared with 
simply  the  keyword  *INCLUDE,  this  keyword  reduces  memory  requirement  for 
trimming by more than 50%.  Levels of CPU time reductions vary, in some cases more 
than 50%. 
Performance Improvements 
Roof 
Hood 
Inr 
B-Plr 
Fender 
BSA 
Otr 
Door 
Otr 
Wheel 
House 
(2 in 1) 
Boxside
Otr 
#Element 
410810 
1021171  351007 
189936 
380988 
315556 
261702 
1908369
CPU 
old 
7m26s 
10m20s  3m11s 
2m6s 
5m45s 
4m27s 
2m52s 
27m31s 
new  4m 
9m18s 
2m56s 
1m22s 
4m54s 
3m35s 
2m30s 
13m59s 
Memory 
(MW) 
old 
282 
new  112 
616 
383 
221 
117 
119 
50 
233 
130 
217 
114 
157 
1150 
75 
539 
Revision information: 
This feature is available in LS-DYNA Revision 62207 or later releases, where the output 
of strain tensors for the shells is included.  Prior Revisions do not include strain tensors 
for the shells.
*INCLUDE_UNITCELL 
Purpose:  This card creates a unit cell model with periodic boundary conditions using 
*CONSTRAINED_MULTIPLE_GLOBAL. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME 
C 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
INPT 
OUPT 
NEDOF 
Type 
Default 
Remarks 
  Card 3 
Variable 
I 
0 
1 
1 
DX 
Type 
F 
I 
0 
2 
DY 
F 
I 
0 
2 
3 
DZ 
F 
Default 
1.0 
1.0 
1.0 
4 
5 
6 
7 
8 
NEX 
NEY 
NEZ 
NNPE 
I 
1 
I 
1 
I 
1 
I
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NOFF 
EOFF 
PNM 
Type 
I 
I 
I 
Default 
none 
none 
none 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CNX 
CNY 
CNZ 
Type 
I 
I 
I 
Default 
none 
none 
none 
Node ID Cards.  Input is terminated at the next keyword (“*”) card 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ECNX 
ECNY 
ECNZ 
Type 
I 
I 
I 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
FILENAME 
Name of the file containing the information of unit cell.  
INPT 
Type of input 
EQ.0:  read  *NODE  information  from  the  include  file  and  add
periodic boundary conditions to the include file. 
EQ.1:  create a unit cell mesh with periodic boundary conditions,
and output to the include file.
VARIABLE   
DESCRIPTION 
OUPT 
Type of output 
EQ.1:  create  a  new  main  keyword  file  where  the  keyword  *IN-
CLUDE_UNITCELL  is  replaced  by  *INCLUDE  with  the
include file name. 
NEDOF 
Number of extra nodal degrees of freedom (DOFs) for user-defined
element.  In the current implementation, the limit of NEDOF is 15. 
DX 
DY 
DZ 
NEX 
NEY 
NEZ 
NNPE 
Defines the 𝑥-dimension of unit cell. 
Defines the 𝑦-dimension of unit cell.  
Defines the 𝑧-dimension of unit cell.  
Defines number of elements along 𝑥-direction. 
Defines number of elements along 𝑦-direction. 
Defines number of elements along 𝑧-direction. 
Defines number of nodes per element.  The current implementation
supports only 4-node tetrahedron or 8-node hexahedron elements. 
NOFF 
Defines offset of nodal IDs. 
EOFF 
PNM 
CNX 
CNY 
CNZ 
ECNX 
ECNY 
Defines offset of elemental IDs. 
Defines part ID. 
Defines  nodal  ID  of  the  1st  control  point  for  the  constraint  in  𝑥
direction. 
Defines  nodal  ID  of  the  2nd  control  point  for  the  constraint  in  𝑦
direction. 
Defines  nodal  ID  of  the  3rd  control  point  for  the  constraint  in  𝑧
direction. 
Defines  nodal  ID  of  extra  control  point  for  the  constraint  in  𝑥
direction of 3 extra nodal DOFs. 
Defines  nodal  ID  of  extra  control  point  for  the  constraint  in  𝑦
direction of 3 extra nodal DOFs.
DESCRIPTION 
Defines  nodal  ID  of  extra  control  point  for  the  constraint  in  𝑧
direction of 3 extra nodal DOFs. 
  VARIABLE   
ECNZ 
Remarks: 
1. 
Include File Field.  If INPT=0, the geometry and discretization information of 
unit cell are from the include file.  In this case, the parameters in cards 3 and 4 
are ignored. 
2.  Extra Degrees of Freedom.  The extra degrees of freedom (DOFs) specified by 
NEDOF>0 are represented by extra nodes with regular 𝑥, 𝑦 and 𝑧 DOFs.  When 
NEDOF=7, for example, the following chart shows the mapping from the extra 
DOFs to the regular ones of extra nodes: 
Extra Node # 
Extra DOFs 
Regular DOFs 
1 
2 
3 
1 
2 
3 
4 
5 
6 
7 
𝑥 
𝑦 
𝑧 
𝑥 
𝑦 
𝑧 
𝑥 
In this case, 3  control points for 𝑥, 𝑦, and 𝑧 directions, respectively, need to be 
defined for each extra node.
The keyword *INITIAL provides a way of initializing velocities and detonation points.  
The keyword control cards in this section are defined in alphabetical order: 
*INITIAL_AIRBAG_PARTICLE_POSITION 
*INITIAL_ALE_MAPPING 
*INITIAL_AXIAL_FORCE_BEAM 
*INITIAL_CONTACT_WEAR 
*INITIAL_DETONATION 
*INITIAL_EOS_ALE 
*INITIAL_FATIGUE_DAMAGE_RATIO 
*INITIAL_FIELD_SOLID 
*INITIAL_FOAM_REFERENCE_GEOMETRY 
*INITIAL_GAS_MIXTURE 
*INITIAL_HYDROSTATIC_ALE 
*INITIAL_IMPULSE_MINE 
*INITIAL_INTERNAL_DOF_SOLID_{OPTION} 
*INITIAL_LAG_MAPPING 
*INITIAL_MOMENTUM 
*INITIAL_PWP_DEPTH 
*INITIAL_STRAIN_SHELL_{OPTION} 
*INITIAL_STRAIN_SOLID_{OPTION} 
*INITIAL_STRAIN_TSHELL 
*INITIAL_STRESS_BEAM 
*INITIAL_STRESS_DEPTH 
*INITIAL_STRESS_SECTION
*INITIAL_STRESS_SOLID 
*INITIAL_STRESS_SPH 
*INITIAL_STRESS_TSHELL 
*INITIAL_TEMPERATURE_{OPTION} 
*INITIAL_VEHICLE_KINEMATICS 
There  are  two  alternative  sets  of  keywords  for  setting  initial  velocities.    Cards 
from one set cannot be combined with cards from the other.  Standard velocity 
cards: 
*INITIAL_VELOCITY 
*INITIAL_VELOCITY_NODE 
*INITIAL_VELOCITY_RIGID_BODY 
Alternative initial velocity cards supporting initial rotational about arbitrary axes 
and start times.  Alternative velocity cards: 
*INITIAL_VELOCITY_GENERATION 
*INITIAL_VELOCITY_GENERATION_START_TIME 
*INITIAL_VOID_{OPTION} 
*INITIAL_VOLUME_FRACTION 
*INITIAL_VOLUME_FRACTION_GEOMETRY
*INITIAL_AIRBAG_PARTICLE_POSITION 
Purpose:    This  card  initializes  the  position  of  CPM  initial  air  particle  to  the  location 
specified. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Bag_ID 
Type 
I 
Default 
none 
Particle Cards.  The ith card specifies the location of the ith particle.  LS-DYNA expects 
one card for each particle, if fewer cards are supplied the coordinates will be reused and 
particles may share the same location at the beginning of the simulation. 
5 
6 
7 
8 
Card 
1 
Variable 
Type 
8x 
Default 
2 
X 
F 
3 
Y 
F 
4 
Z 
F 
  VARIABLE   
DESCRIPTION
Bag_ID 
Airbag ID defined in *AIRBAG_PARTICLE_ID card 
X 
Y 
Z 
𝑥 coordinate 
𝑦 coordinate 
𝑧 coordinate
*INITIAL_ALE_MAPPING 
Purpose:    This  card  initializes  the  current  ALE  run  with  data  from  the  last  cycle  of  a 
previous  ALE  run.    Data  are  read  from  a  mapping  file  specified  by  “map=”  on  the 
command line .  To map data histories (not just the last cycle) to a region 
of selected elements see *BOUNDARY_ALE_MAPPING. 
The following transitions are allowed: 
1D → 2D 
1D → 3D 
2D → 2D 
2D → 3D 
3D → 3D 
3D → 2D 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
TYP 
AMMSID 
Type 
I 
I 
I 
Default 
none 
none 
none 
  Card 2 
Variable 
1 
XO 
Type 
F 
2 
YO 
F 
3 
ZO 
F 
4 
5 
6 
7 
8 
VECID 
ANGLE 
I 
F 
Default 
0.0 
0.0 
0.0 
none 
none 
  VARIABLE   
DESCRIPTION
PID 
TYP 
Part ID or part set ID. 
Type of “PID” : 
EQ.0: part set ID (PSID). 
EQ.1: part ID (PID). 
AMMSID 
Set  ID  of  ALE  multi-material  groups  defined  in  *SET_MULTI-
MATERIAL_GROUP.  See Remark 1. 
XO 
Origin position in global 𝑥-direction.  See Remarks 2 and 5.
VARIABLE   
DESCRIPTION
Origin position in global 𝑦-direction.  See Remarks 2 and 5. 
Origin position in global 𝑧-direction.  See Remarks 2 and 5. 
ID  of  the  symmetric  axis  defined  by  *DEFINE_VECTOR.    See 
Remarks 3 and 5. 
Angle  of  rotation  in  degrees  around  an  axis  defined  by  *DE-
FINE_VECTOR for the 3D to 3D mapping.  See Remark 4. 
YO 
ZO 
VECID 
ANGLE 
Remarks: 
1.  Mapping  of  Ale  Multi-Material  Groups.    The  routines  of  this  card  need  to 
know which mesh will be initialized with the mapping data, and more specifi-
cally,  which  multi-material  groups.    The first  two  fields,  PID,  and  TYP,  define 
the mesh.  The third field, AMMSID, refers to a multi-material group list ID; see 
the  *SET_MULTI-MATERIAL_GROUP_LIST  card.    The  group  list  AMMSID 
should  have  as  many  elements  as  there are groups  in  the  previous  calculation 
.  
Example:  If the previous model has 3 groups, the current one has 5 groups and 
the following mapping is wanted. 
Group 1 from the previous run → Group 3 in the current run
Group 2 from the previous run → Group 5 in the current run
Group 3 from the previous run → Group 4 in the current run
The  *SET_MULTI-MATERIAL_GROUP_LIST card should be set as follows: 
*SET_MULTI-MATERIAL_GROUP_LIST 
300 
3,5,4 
In special cases, a group can be replaced by another.  If the group 4 in the pre-
vious example should be replaced by the group 3, the keyword setup would be 
modified to have -3 instead of 4.  The minus sign is a way for the code to know 
that the replacing group (-3 replaces 4) is a complement of the group 3: 
*SET_MULTI-MATERIAL_GROUP_LIST 
300 
3,5,-3 
2.  Coordinate  System  Origin.    The  location  to  which  the  data  is  mapped  is 
controlled by the origin of the coordinate system (XO, YO, ZO).
3.  Symmetry Axis.  For a mapping file created by a previous asymmetric model, 
the symmetric axis orientation in the current model is specified by VECID.  For 
a mapping file created by a 3D or 1D spherical model, the vector VECID is read 
but ignored.  For a 3D to 3D mapping the vector is used if the parameter AN-
GLE is defined .  
4.  Rotating 3D Data Onto a 3D calculation.  For a mapping from a previous 3D 
run to a current 3D model the previous 3D data will be rotated about the vector, 
VECID, through an angle specified in the ANGLE field.  
5.  Plain Strain, and 3D to 2D.  The definitions of X0, Y0, Z0 and VECID change in 
the case of the following mappings: 
a)  plain strain 2D (ELFORM = 13 in *SECTION_ALE2D) to plain strain 2D 
b)  plain strain 2D to 3D 
c)  3D to 2D  
While, VECID still defines the y-axis in the 2D domain, the 3 first parameters in 
*DEFINE_VECTOR,  additionally,  define  the  location  of  the  origin.    The  3  last 
parameters  defines  a  position  along  the  y-axis.    For  this  case  when  2D  data  is 
used in a 3D calculation the point X0, Y0, Z0 together with the vector, VECID, 
define the plane. 
6.  Mapping File.  Including the command line argument “map=” will invoke the 
creation of a mapping file.  When the keyword INITIAL_ALE_MAPPING is not 
in  the  input  deck,  but  the  argument  “map=”  is  present  on  the  command  line, 
the  ALE  data  from  the  last  cycle  is  written  in  the  mapping  file.    This  file  con-
tains the following nodal and element data: 
•  nodal coordinates (last step) 
•  nodal velocities 
•  part ids 
•  element connectivities 
•  element centers 
•  densities 
•  volume fractions 
•  stresses 
•  plastic strains 
•  internal energies 
•  bulk viscosities
*INITIAL 
Chained  Mappings.    To  chain  mapping  operations  so  that  LS-DYNA  both 
reads and writes a mapping file the command line argument “map1=” is neces-
sary.    If  the  keyword  INITIAL_ALE_MAPPING  is  in  the  input  deck  and  the 
prompt “map=” is in the command line, the ALE data is read from the mapping 
file defined by “map=” to initialize the run.  Data from the last cycle are written 
in the mapping file defined by “map1=”.
*INITIAL_AXIAL_FORCE_BEAM 
Purpose:    Initialize  the  axial  force  resultants  in  beam  elements  that  are  used  to  model 
bolts.  This option works with *MAT_SPOTWELD with beam type 9, a Hughes-Liu type 
beam. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BSID 
LCID 
SCALE 
KBEND 
Type 
I 
I 
F 
Default 
none 
none 
1.0 
I 
0 
  VARIABLE   
DESCRIPTION
BSID 
LCID 
Beam set ID. 
Load curve ID defining preload force versus time.  When the load
curve  ends  or  goes  to  zero,  the  initialization  is  assumed  to  be
completed.  See Remark 2 below. 
SCALE 
Scale factor on load curve. 
KBEND 
Bending stiffness flag 
EQ.0:  Bending stiffness is negligible since all integration points
are assigned the same axial stress 
EQ.1:  Bending  stiffness  is  retained  by  keeping  the  axial  stress 
gradient 
Remarks: 
1.  Damping.    To  achieve  convergence  during  explicit  dynamic  relaxation,  the 
application of the damping options is very important.  If contact is active, con-
tact damping is recommended with a value between 10-20 percent.  Additional 
damping,  via  the  option  DAMPING_PART_STIFFNESS  also  speeds  conver-
gence  where  a  coefficient  of  0.10  is  effective.    If  damping  is  not  used,  conver-
gence may not be possible. 
2.  Ramping.    When  defining  the  load  curve,  LCID,  a  ramp  starting  at  the  origin 
should be used to increase the force to the desired value.  The time duration of 
the  ramp  should  produce  a  quasistatic  response.    When  the  end  of  the  load
curve  is  reached,  or  when  the  value  of  the  load  decreases  from  its  maximum 
value, the initialization stops.  If the load curve begins at the desired force val-
ue,  i.e.,  no  ramp,  convergence  will  take  much  longer,  since  the  impulsive  like 
load created by the initial force can excite nearly every frequency in the struc-
tural system where force is initialized.
*INITIAL_CONTACT_WEAR 
Purpose:  Initialize contact wear for simulation of wear processes, define as many cards 
as necessary. 
  Card 1 
1 
2 
3 
4 
Variable 
CID 
NID 
WDEPTH 
NX 
Type 
I 
I 
F 
F 
5 
NY 
F 
6 
NZ 
F 
7 
8 
ISEQ 
NCYC 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
CID 
NID 
Contact Interface ID.   
Node ID. 
WDEPTH 
Wear depth, in units of length. 
NX, NY, NZ 
Direction vector for wear, internally normalized. 
Simulation sequence number for the entire process. 
The  wear  on  this  card  will  be  processed  NCYC  times  to  modify
the worn geometry.  This is to say that one LS-DYNA simulation 
is used to predict the wear for NCYC repetitions of the process, in 
order  to  save  simulation  time.    This  number  should  be  chosen 
with care, a negative number means that LS-DYNA will not apply 
this card, see remarks below. 
ISEQ 
NCYC 
Remarks: 
This  is  a  card  that  is  not  supposed  to  be  manually  inserted,  but  is  automatically 
generated  by  LS-DYNA  when  simulating  wear  processes,  see  *CONTACT_ADD_-
WEAR  and  parameters  NCYC  on  *INTERFACE_SPRINGBACK_LSDYNA  and 
SPR/MPR on *CONTACT.  A sequence of identical simulations, except for perturbation 
of the geometry of certain components due to wear, is undertaken.  For a given contact 
interface  and  node  ID,  the  corresponding  node  is  perturbed  by  the  wear  depth  in  the 
direction of wear.  If the cycle number NCYC is negative, this means that the geometry
has been already processed in LS-PrePost and the card is ignored by LS-DYNA, and if a 
node appears multiple times the wear from the individual sequences is accumulated.
*INITIAL_CRASHFRONT 
Purpose:  To define initial crashfront node set for materials supporting crashfront. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
STYPE 
Type 
I 
Default 
none 
I 
0 
  VARIABLE   
DESCRIPTION
SID 
Crash front node set ID for initial crashfront nodes. 
STYPE 
ID type of SID: 
EQ.0:  segment set ID, 
EQ.1:  shell element set ID, 
EQ.2:  part set ID, 
EQ.3:  part ID, 
EQ.4:  node set ID. 
Remarks: 
Material models 17, 54, 55, 58, 169, 261, and 262 reduce material strength in crashfront 
elements.  This keyword defines the initial crashfront nodes, and all elements connected 
to these nodes are initialized as crashfront elements with reduced strength.
*INITIAL 
Purpose:  Define points to initiate the location of high explosive detonations in part ID’s 
which  use    *MAT_HIGH_EXPLOSIVE_BURN  (*MAT_008).    Also  see  *CONTROL_EX-
PLOSIVE_SHADOW.  If no *INITIAL_DETONATION is defined, detonation occurs in 
all the high explosive elements at time = 0. 
6 
7 
8 
  Card 1 
1 
Variable 
PID 
Type 
I 
2 
X 
F 
3 
Y 
F 
4 
Z 
F 
Default 
all HE 
0. 
0. 
0. 
5 
LT 
F 
0. 
Accoustic Boundary Card.  Additional card for PID = -1.  
  Card 2 
1 
2 
Variable 
PEAK 
DECAY 
Type 
Remark 
F 
1 
F 
1 
3 
XS 
F 
4 
YS 
F 
5 
ZS 
F 
6 
NID 
I 
7 
8 
  VARIABLE   
PID 
DESCRIPTION
Part ID of the high explosive to be lit, except in the case where the
high  explosive  is  modeled  using  an  ALE  formulation,  in  which
case  PID  is  the  part  ID  of  the  mesh  where  the  high  explosive
material to be lit initially resides.  However, two other options are 
available: 
EQ.-1: an  acoustic  boundary,  also,  *BOUNDARY_USA_SUR-
FACE, 
EQ.0:  all high explosive materials are considered. 
X 
Y 
𝑥-coordinate of detonation point, see Figure 23-1. 
𝑦-coordinate of detonation point.
Z 
LT 
*INITIAL_DETONATION 
DESCRIPTION
𝑧-coordinate of detonation point. 
Lighting  time  for  detonation  point.    This  time  is  ignored  for  an
acoustic boundary. 
PEAK 
Peak pressure, po, of incident pressure pulse, see remark below. 
DECAY 
Decay constant, τ 
XS 
YS 
ZS 
𝑥-coordinate of standoff point, see Figure 23-1. 
𝑦-coordinate of standoff point 
𝑧-coordinate of standoff point 
NID 
Reference node ID near structure
Pressure profile at
standoff point
Standoff point
Structure
Reference node where pressure
begins at t=0. This node is typically
one element away from the
structure.
Acoustic mesh boundary
is treated as a transmitting
boundary.
Detonation point
Figure  23-1.    Initialization  of  the  initial  pressures  due  to  an  explosive
disturbance  is  performed  in  the  acoustic  media.    LS-DYNA  automatically
determines the acoustic mesh boundary and applies the pressure time history
to  the  boundary.    This  option  is  only  applicable  to  the  acoustic  element
formulation, see *SECTION_SOLID. 
Remarks: 
For solid elements (not acoustic) two options are available.  If the  control card option, 
*CONTROL_EXPLOSIVE_SHADOW,  is  not  used  the  lighting  time  for  an  explosive 
element  is  computed  using  the  distance  from  the  center  of  the  element  to  the  nearest 
detonation point, 𝐿𝑑; the detonation velocity, 𝐷; and the lighting time for the detonator, 
𝑡𝑑: 
𝑡𝐿 = 𝑡𝑑 +
𝐿𝑑
. 
The detonation velocity for this default option is taken from the element whose lighting 
time  is  computed  and  does  not  account  for  the  possibilities  that  the  detonation  wave 
may travel through other explosives with different detonation velocities or that the line 
of sight may pass outside of the explosive material. 
If the control card option, *CONTROL_EXPLOSIVE_SHADOW, is defined, the lighting 
time is based on the shortest distance through the explosive material.  If inert obstacles 
exist  within  the  explosive  material,  the  lighting  time  will  account  for  the  extra  time 
required for the detonation wave to travel around the obstacles.  The lighting times also
automatically  accounts  for  variations  in  the  detonation  velocity  if  different  explosives 
are used.  No additional input is required for this option but care must be taken when 
setting up the input.  This option works for two and three-dimensional solid elements.  
It is recommended that for best results: 
1.  Keep  the  explosive  mesh  as  uniform  as  possible  with  elements  of  roughly  the 
same dimensions. 
2. 
Inert  obstacle  such  as  wave  shapers  within  the  explosive  must  be  somewhat 
larger  than  the  characteristic  element  dimension  for  the  automatic  tracking  to 
function properly.  Generally, a factor of two should suffice.  The characteristic 
element  dimension  is  found  by  checking  all  explosive  elements  for  the  largest 
diagonal. 
3.  The  detonation  points  should  be  either  within  or  on  the  boundary  of  the 
explosive.  Offset points may fail to initiate the explosive.  When LT is nonzero, 
the detonation point is fixed to the explosive material at t = 0 and moves as the 
explosive material moves prior to detonation. 
4.  Check  the  computed  lighting  times  in  the  post  processor  LS-PREPOST.    The 
lighting times may be displayed at time = 0., state 1, by plotting component 7 (a 
component normally reserved for plastic strain) for the explosive material.  The 
lighting  times  are  stored  as  negative  numbers.    The  negative  lighting  time  is 
replaced by the burn fraction when the element ignites. 
Line  detonations  may  be  approximated  by  using  a  sufficient  number  of  detonation 
points  to  define  the  line.    Too  many  detonation  points  may  result  in  significant 
initialization cost. 
The pressure versus time curve for the acoustic option is defined by: 
𝑝(𝑡) = 𝑝𝑜𝑒− 𝑡
𝜏.
*INITIAL 
Purpose:    This  card  initializes  the  pressure  in  ALE  elements  that  have  materials  with 
*EOS. 
  Card 1 
Variable 
1 
ID 
2 
3 
TYP 
MMG 
Type 
I 
I 
I 
4 
E0 
F 
5 
V0 
F 
6 
P0 
F 
7 
8 
Default 
none 
none 
none 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
ID 
TYP 
Part ID or part set ID or element set ID. 
Type of “ID”: 
EQ.0: part set ID. 
EQ.1: part ID. 
EQ.2: element  set  ID  (*SET_BEAM  in  1D,  *SET_SHELL  in  2D, 
*SET_SOLID in 3D). 
MMG 
Specifies the multi-material group. 
GT.0: ALE multi-material group. 
LT.0:  Set  ID  of  ALE  multi-material  groups  defined  in  *SET_-
MULTI-MATERIAL_GROUP. 
Initial  internal  energy  per  reference  volume  unit  (as  defined  in
*EOS).  See Remark 1. 
Initial relative volume (as defined in *EOS).  See Remark 1. 
Initial pressure.  See Remark 2. 
E0 
V0 
P0 
Remarks: 
1. 
Initialization with Volume and Energy.  For most *EOS, E0 and V0 should be 
used  to  initialize  the  pressure.    If  only  the  internal  energy  is  initialized,  V0 
should be 1.0 ( If V0 = 0.0, E0 will not be applied).
2. 
Initial Pressure with Derived Volume and Energy.  For *EOS_001, *EOS_004 
and *EOS_006, the initial pressure P0 can be input directly.  An iterative meth-
od will compute the initial internal energy and relative volume.  This approach 
is applied if E0 = 0.0 and V0 = 0.0.
*INITIAL_FATIGUE_DAMAGE_RATIO_{OPTION} 
Available options include: 
<BLANK> 
BINARY 
Purpose:    This  card  sets  initial  damage  ratio  for  fatigue  analysis.    The  initial  damage 
ratio  may  come  from  the  previous  loading  cases.    The  initial  damage  ratio  can  be 
defined by user directly, or can be extracted from existing binary database like D3FTG 
(using the option BINARY). 
Card 1 for no option, <BLANK>. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID/SID 
PTYP 
DRATIO 
Type 
I 
Default 
none 
I 
0 
F 
0.0 
Card 1 for option BINARY. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME 
C 
d3ftg 
  VARIABLE   
DESCRIPTION
PID/SID 
Part ID or part set ID for which the initial damage ratio is defined.
PTYP 
Type of PID/SID: 
EQ.0: part ID. 
EQ.1: part set ID.
*INITIAL_FATIGUE_DAMAGE_RATIO 
DESCRIPTION
DRATIO 
Initial damage ratio. 
FILENAME 
Path  and  name  of  existing  binary  database 
information. 
for 
fatigue 
Remarks: 
1.  The  card  works  for  both  time  domain  fatigue  and  frequency  domain  fatigue 
problems. 
2.  Card  1  can  be  repeated  if  the  model  has  initial  damage  ratio  coming  from 
multiple loading cases.
*INITIAL 
Purpose:  This keyword is a simplified version of *INITIAL_STRESS_SOLID which can 
be  used  with  hyperelastic  materials.    The  keyword  is  used  for  history  variable  input.  
Data  is  usually  in  the  form  of  the  eigenvalues  of  diffusion  tensor  data.    These  are 
expressed  in  the  global  coordinate  system.    The  input  deck  takes  the  following 
parameters: 
NOTE:  As  of  LS-DYNA  R5  in  all  contexts,  other  than 
*MAT_TISSUE_DISPERSED, this keyword is depre-
cated  (and  disabled).    For  all  other  materials  this 
keyword  has  been  superceded  by  *INITIAL_-
STRESS_SOLID. 
Include  as  many  pairs  of  cards  1  and  2  as  necessary.    This  input  ends  at  the  next 
keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EID 
NINT 
NHISV 
Type 
I 
I 
Default 
none 
none 
  Card 2 
1 
2 
I 
0 
3 
4 
5 
6 
7 
8 
Variable 
FLD1 
FLD2 
FLD3 
FLD4 
FLD5 
FLD6 
FLD7 
FLD8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
  VARIABLE   
DESCRIPTION
EID 
NINT 
Element ID 
Number  of  integration  points  (should  correspond  to  the  solid
element formulation).
NHISV 
*INITIAL_FIELD_SOLID 
DESCRIPTION
Number  of  field  variables.      If  NHISV  exceeds  the  number  of
integration  point  field  variables  required  by  the  constitutive
model, only the number required is output; therefore, if in doubt,
set NHISV to a large number. 
FLDn 
Data  for  the  nth  field  (history)  variable.    NOTE  that  *MAT_TIS-
SUE_DISPERSED only use FLD1 to FLD3 since NHISV = 3. 
Remarks: 
Add as many cards as necessary.  The keyword input ends when next keyword appears 
(next *).  For example for two elements it can look as: 
*INITIAL_FIELD_SOLID 
$EID      NINT    NHISV 
    1        1        3 
$FLD1     FLD2     FLD3 
  0.1      0.8      0.1 
$EID      NINT    NHISV 
    2        1        3 
$FLD1     FLD2     FLD3 
  0.3      0.2      0.5
*INITIAL_FOAM_REFERENCE_GEOMETRY_OPTION 
Available options include: 
RAMP 
Purpose:  The reference configuration allows stresses to be initialized (via REF in *MAT) 
in the following hyperelastic material models: 2, 5, 7, 21, 23, 27, 31, 38, 57, 73, 77, 83, 132, 
179,  181,  183,  and  189.    Supported  solid  elements  are  the  constant  stress  hexahedron 
(#1),  the  fully  integrated  S/R  hexahedron  (#2),  the  tetrahedron  (#10),  and  the 
pentahedron (#15). 
To  use  this  option,  the  geometry  of  the  foam  material  is  defined  in  a  deformed 
configuration.    The  stresses  in  the  low  density  foam  then  depend  only  on  the 
deformation gradient matrix 𝐹𝑖𝑗: 
𝐹𝑖𝑗 =
∂𝑥𝑖
∂𝑋𝑗
where  𝑥𝑖  is  the  deformed  configuration  and  𝑋𝑗  is  the  undeformed  configuration.    By 
using this option, dynamic relaxation can be avoided once a deformed configuration is 
obtained usually on the first run of a particular problem. 
Optional RAMP Card.  Additional optional card for the option of RAMP. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NDTRRG 
Type 
Default 
I
Include as many cards as necessary.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
NID 
Type 
I 
X 
F 
Default 
none 
0. 
Y 
F 
0. 
Z 
F 
0. 
Remarks 
  VARIABLE   
NDTRRG 
DESCRIPTION
Number of time steps taken for an element to restore its reference
geometry.  Definition of NDTRRG allows an element to ramp up
to its reference shape in NDTRRG time steps.  Currently ls-dyna 
uses only one NDTRRG and applies it to all foam materials with
reference  geometries.   If  more  than  one  NDTRRG  is  defined,  the
latter defined one will replace the previously define one.  
NID 
Node number 
X 
Y 
Z 
𝑥 coordinate in reference configuration 
𝑦 coordinate in reference configuration 
𝑧 coordinate in reference configuration
*INITIAL 
Purpose:  This command is used to specify (a) which ALE multi-material groups may be 
present  inside  an  ALE  mesh  set  at  time  zero,  and  (b)  the  corresponding  reference  gas 
temperature and density which define the initial thermodynamic state of the gases.  The 
order of the species in the gas mixture corresponds to the order of different gas species 
defined in the associated *MAT_GAS_MIXTURE card.  This card must be used together 
with a *MAT_GAS_MIXTURE (or equivalently, a *MAT_ALE_GAS_MIXTURE) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
STYPE 
MMGID 
TEMP 
Type 
I 
Default 
none 
  Card 2 
1 
I 
0 
2 
I 
F 
none 
none 
3 
4 
5 
6 
7 
8 
Variable 
RO1 
RO2 
RO3 
RO4 
RO5 
RO6 
RO7 
RO8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
SID 
DESCRIPTION
Set  ID  for  initialization.    This  SID  defines  the  ALE  mesh  within
which  certain  ALE  multi-material  group(s)  may  be  present  at 
𝑡 = 0. 
STYPE 
Set type for the SID above: 
EQ.0: SID is a part set ID 
EQ.1: SID is a part ID 
MMGID 
ALE Multi-material group ID of the material that may be present 
at t = 0 in the ALE mesh set defined by SID.
Initial  static  temperature  of  the  gas  species  occupying  the  ALE
mesh.    Note  that  all  species  in  the  mixture  are  assumed  to  be  in
thermal equilibrium (having the same 𝑇). 
Initial  densities  of  the  ALE  material(s)  which  may  be  occupying
some  region  (or  all)  of  the  aforementioned  ALE  mesh,  for  up  to
eight  different  gas  species.    The  order  of  the  density  input
corresponds  to  the  order  of  the  materials  defined  in  associated 
*MAT_GAS_MIXTURE card. 
*INITIAL 
  VARIABLE   
TEMP 
RO1-RO8 
Remarks: 
1.  Please see the example under the *MAT_GAS_MIXTURE card definition for an 
application of the *INITIAL_GAS_MIXTURE card. 
2.  The  temperature  is  assumed  to  be  the  initial  temperature  which  together  with 
the gas density, will define the initial pressure of the gas species via the perfect 
gas law, 
The user should manually check the initial pressure for consistency. 
𝑃|𝑡=0 = 𝜌∣𝑡=0(𝐶𝑃 − 𝐶𝑉)𝑇|𝑡=0. 
3.  Given an ALE mesh, this mesh may initially be occupied by one or more ALE 
multi-material  groups  (AMMG).    For  example,  a  background  ALE  mesh  (H1) 
containing AMMG 1 may be partially filled with AMMG 2 via the volume fill-
ing command *INITIAL_VOLUME_FRACTION_GEOMETRY.  Then there are 2 
AMMGs to be initialized for this mesh H1.  The commands look like the follow-
ing. 
$--------------------------------------------------------------------------- 
$ One card is defined for each AMMG that will occupy some elements of a mesh 
set 
*INITIAL_GAS_MIXTURE 
$      SID     STYPE     MMGID        T0 
         1         1         1    298.15 
$     RHO1      RHO2      RHO3      RHO4      RHO5      RHO6      RHO7      
RHO8 
    1.0E-9 
*INITIAL_GAS_MIXTURE 
$      SID     STYPE     MMGID        T0 
         1         1         2    298.15 
$     RHO1      RHO2      RHO3      RHO4      RHO5      RHO6      RHO7     
RHO8 
    1.2E-9 
$---------------------------------------------------------------------------
*INITIAL 
Purpose:  When an ALE model contains one or more regular (not reservoir-type) ALE 
parts  (ELFORM = 11  and  AET = 0),  this  command  may  be  used  to  initialize  the 
hydrostatic  pressure  field  in  the  regular  ALE  domain  due  to  gravity.    The  *LOAD_-
BODY_(OPTION) keyword must be defined. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ALESID 
STYPE 
VECID 
GRAV 
PBASE 
Type 
I 
Default 
none 
I 
0 
I 
none 
I 
0 
I 
0 
Multi-material  Layers  Group  Cards.    Repeat  card  2  as  many  times  as  the  number  of 
AMMG layers present in the model.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID 
MMGBLO 
Type 
I 
I 
Default 
none 
none 
  VARIABLE   
ALESID 
DESCRIPTION
ALESID  is  a  set  ID  defining  the  ALE  domain/mesh  whose
hydrostatic  pressure  field  due  to  gravity  is  being  initialized  by
this keyword. See Remark 2 and 4. 
STYPE 
ALESID set type.  See Remark 4. 
EQ.0: Part set ID (PSID), 
EQ.1: Part ID (PID), 
EQ.2: Solid set ID (SSID). 
VECID 
Vector ID of a vector defining the direction of gravity.
GRAV 
PBASE 
*INITIAL_HYDROSTATIC_ALE 
DESCRIPTION
Magnitude  of  the  Gravitational  acceleration.    For  example,  in
metric units the value is usually set to 9.80665 m/s2. 
Nominal  or  reference  pressure  at  the  top  surface  of  all  fluid
layers.    By  convention,  the  gravity  direction  points  from  the  top
layer to the bottom layer.  Each fluid layer must be represented by
an  ALE  multi-material  group  ID  (AMMGID  or  MMG).    See
Remark 1. 
NID 
Node ID defining the top of an ALE fluid (AMMG) layer. 
MMGBLO 
AMMG  ID  of  the  fluid  layer immediately  below  this  NID.    Each
node  is  defined  in  association  with  one  AMMG  layer  below  it.
See Remark 3. 
Remarks: 
1.  Pressure in Multi-Layer Fluids.  For models using multi-layer ALE Fluids the 
pressure at the top surface of the top fluid layer is set to PBASE and the hydro-
static pressure is computed as following 
𝑁layers
𝑃 = 𝑃base + ∑ 𝜌𝑖𝑔ℎ𝑖
 . 
𝑖=1
2.  Limitations  on  Element  Formulation.    The  keyword  applies  only  to  the 
regular  ALE  parts  with  ELFORM = 11  and  AET = 0  on  the  *SECTION_SOLID 
and  *SECTION_ALE2D  cards  (not  reservoir-type).    This  keyword  cannot  be 
used to initialize reservoir-type ALE parts (AET = 4).  Also, ramping functions 
are  not  supported,  so the  loading  is  done  in  one  step  at 𝑡 = 0.    For  initializing 
reservoir-type ALE domain, please review the *ALE_AMBIENT_HYDROSTAT-
IC keyword. 
3.  Limitation  on  EOS  Model.    The  keyword  only  supports  *EOS_GRUNEISEN 
and  *EOS_LINEAR_POLYNOMIAL, but only inthe following two cases, 
𝑐4 = 𝑐5 > 0,
𝑐3 = 𝑐4 = 𝑐5 = 𝑐6 = 0,
𝑐1 = 𝑐2 = 𝑐3 = 𝑐6 = 0,
𝐸0 = 0
𝑉0 = 0.
4.  Structured  ALE  usage.      When  used  with  structured  ALE,  PART  and  PART 
set options might not make too much sense.  This is because all elements inside 
a structured ALE mesh are assigned to one single PART ID.  If we want to pre-
scribe  initial  hydrostatic  pressure  for  all  the  elements  inside  the  structured 
mesh,  we  can  certainly  use  that  PART  ID.    But  if  we  only  want  to  do  that  to 
some elements, we have to generate a solid set which contains those structured
ALE elements.  It is done by using the *SET_SOLID_GENERAL keyword with 
SALECPT option.  And then use STTYPE=2 (solid element set ID) option. 
Example: 
Model Summary: Consider a model consisting of 2 ALE parts, air on top of water. 
H1 = AMMG1 = Air part above. 
H2 = AMMG2 = Water part below. 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
$ (non-ambient) ALE materials (fluids) listed from top to bottom: 
$ 
$ NID AT TOP OF A LAYER SURFACE         ALE MATERIAL LAYER BELOW THIS NODE 
$ TOP OF 1st LAYER -------> 1722        ---------------------------------------- 
$                                       Air above   = PID 1 = H1 = AMMG1 (AET=0) 
$ TOP OF 2nd LAYER -------> 1712        ---------------------------------------- 
$                                       Water below = PID 2 = H2 = AMMG2 (AET=0) 
$ BOTTOM ----------------------------------------------------------------------- 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
*INITIAL_HYDROSTATIC_ALE 
$   ALESID     STYPE     VECID      GRAV     PBASE 
        12         0        11   9.80665  101325.0 
$      NID    MMGBLO 
      1722         1 
      1712         2 
*SET_PART_LIST 
        12 
         1         2 
*ALE_MULTI-MATERIAL_GROUP 
         1         1 
         2         1 
*DEFINE_VECTOR 
$      VID        XT        YT        ZT        XH        YH        ZH       CID 
        11       0.0       1.0       0.0       0.0       0.0       0.0 
*DEFINE_CURVE 
         9 
               0.000               0.000 
               0.001               1.000 
              10.000               1.000 
*LOAD_BODY_Y 
$     LCID        SF    LCIDDR        XC        YC        ZC 
         9   9.80665         0       0.0       0.0       0.0 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8
*INITIAL_IMPULSE_MINE 
Purpose:    Apply  initial  velocities  to  the  nodes  of  a  3D  structure  due  to  the  impulse 
imparted  by  the  detonation  of  a  buried  land  mine.    This  feature  is  based  on  the 
empirical model developed by [Tremblay 1998]. 
  Card 1 
1 
Variable 
SSID 
Type 
I 
2 
M 
F 
3 
4 
5 
6 
7 
8 
RHOS 
DEPTH 
AREA 
SCALE 
not used 
UNIT 
F 
F 
F 
F 
Default 
none 
0.0 
0.0 
0.0 
0.0 
1.0 
I 
1 
Remarks 
1 
2 
Either set a heading or delete this row. 
  Card 1 
Variable 
Type 
1 
X 
F 
2 
Y 
F 
3 
Z 
F 
Default 
0.0 
0.0 
0.0 
4 
5 
6 
7 
8 
NIDMC 
GVID 
TBIRTH 
PSID 
SEARCH 
I 
0 
I 
F 
none 
0.0 
I 
0 
F 
0.0 
  VARIABLE   
DESCRIPTION
SSID 
Segment set ID  
MTNT 
RHOS 
DEPTH 
Equivalent mass of TNT . 
Density of overburden soil. 
Burial  depth  from  the  ground  surface  to  the  center  of  the  mine.
This value must be a positive. 
AREA 
Cross sectional area of the mine. 
SCALE 
Scale factor for the impulse.
VARIABLE   
UNIT 
DESCRIPTION
Unit  system.    This  must  match  the  units  used  by  finite  element
model. 
EQ.1: inch, dozen slugs (i.e., lbf × s2/in), second, PSI (default) 
EQ.2: meter, kilogram, second, Pascal 
EQ.3: centimeter, gram, microsecond, megabar 
EQ.4: millimeter, kilogram, millisecond, GPa 
EQ.5: millimeter, metric ton, second, MPa 
EQ.6: millimeter, gram, millisecond, MPa 
X, Y, Z 
𝑥-, 𝑦-, and 𝑧- coordinates of mine center. 
NIDMC 
GVID 
Optional  node  ID  representing  the  mine  center  .    If
defined then X, Y and Z are ignored. 
Vector  ID  representing  the  vertically  upward  direction,  i.e.,
normal to the ground surface . 
TBIRTH 
Birth time.  Impulse is activated at this time. 
Part set ID identifying the parts affected by the mine .  If zero it defaults to the part comprised by the nodes of
the segment set. 
Limit the search depth into the structure.  Initial nodal velocity is
distributed  from  the  segment  to  a  depth  equal  to  the  SEARCH
value.  The value must be positive.  If set to zero the search depth 
is unlimited and extends through the part(s) identified by PSID.  
PSID 
SEARCH 
Remarks: 
1.  Segment normals should nominally point toward the mine. 
2.  The segments should belong to 3D thin shell, solid, or thick shell elements.  This 
feature cannot be applied to 2D geometries. 
3.  Several methods can be used to approximate the equivalent mass of TNT for a 
given  explosive.    One  method  involves  scaling  the  mass  by  the  ratio  of  the 
squares  of  the  Chapman-Jouguet  detonation  velocities  given  by  the  relation-
ship.
z 
GVID 
mine
soil 
(𝑥, 𝑦, 𝑧)
Figure 23-2.  Schematic of the buried mine parameters. 
𝑀TNT = 𝑀
(DCJ)2
(DCJ)TNT
is the Chapman-Jouguet 
where 𝑀TNT is the equivalent TNT mass and (DCJ)TNT
detonation  velocity  of  TNT.    𝑀  and  DCJ  are,  respectively,  the  mass  and  C-J 
velocity of the explosive under investigation.  “Standard” TNT is considered to 
be cast with a density of 1.57gm/cm3 and (DCJ)TNT = 0.693 cm/𝜇sec. 
4.  This  implementation  assumes  the  energy  release  (heat  of  detonation)  for  1 
kilogram of TNT is 4.516 MJ. 
5.  Prediction of the impulse relies on an empirical approach which involves fitting 
curves to experimental results.  The upper error bound is 1.8 times the predict-
ed value and the lower is predicted value divided by 1.8.  Thus, if the predicted 
impulse is 10 kN-seconds then the solution space ranges from 5.6 kN-sec to 18 
kN-sec. 
6.  The computed impulse is valid when the following criteria are met. 
0.106 ≤
6.35 ≤
𝐸 𝐴⁄
𝜌𝑐2𝑧
≤ 1 
≤ 150
0.154 ≤
0 ≤
√𝐴
≤ 4.48 
≤ 19.3 
where, 
𝛿 = the distance from the mine center to the ground surface (DEPTH) 
𝑧 = the vertical distance from the mine center to the target point 
𝐸 = the energy release of the explosive 
𝐴 = the cross-sectional area of the mine (AREA) 
𝜌 = the soil density (RHOS) 
𝑐 = the wave speed in the soil 
𝑑 = the lateral distance from the mine center to the target point. 
See Figure 23-2. 
References: 
Tremblay,  J.E.,  “Impulse  on  Blast  Deflectors  from  a  Landmine  Explosion,”  DRDC 
Valcartier, DREV-TM-9814, (1998).
*INITIAL_INTERNAL_DOF_SOLID_OPTION 
Available Options Include: 
TYPE3 
TYPE4 
Purpose:  Initialize the internal degrees of freedom for solid element types 3 and 4. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LID 
Type 
I 
Default 
none 
Value Cards.  Include 12 cards TYPE3 and 6 cards for TYPE4. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VALX 
VALY 
VALZ 
Type 
F 
F 
F 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION
LID 
VALX 
VALY 
VALZ 
Element ID.   
𝑥 component of internal degree of freedom. 
𝑦 component of internal degree of freedom. 
𝑧 component of internal degree of freedom.
Remarks: 
1.  The internal degrees of freedom are specified in terms of the displacements of 
the corresponding mid-side nodes of the 20 node hex and the 10 node tetrahe-
dron that are the basis of the type 3 and 4 solid elements, respectively.
The available options are 
<BLANK> 
WRITE 
*INITIAL_LAG_MAPPING 
Purpose:  This card initializes a 3D Lagrangian calculation with data from the last cycle 
of a preceding 2D or 3D Lagrangian calculation. 
In its *INITIAL_LAG_MAPPING form (<BLANK> option), this keyword causes data to 
be  read  in  from  a  mapping  file;  while,  with  the  WRITE  active  this  card  is  used  to  set 
which  parts  are  written  to  the  mapping  file.    The  mapping  file’s  filename  is  specified 
using the “lagmap=” command line argument . 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SETID 
Type 
I 
Default 
none 
Card 2.  Additional card for <BLANK> keyword option. 
4 
5 
6 
7 
8 
VECID 
ANGLE  NELANGL 
  Card 2 
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
3 
ZP 
F 
I 
F 
I 
0 
Default 
0.0 
0.0 
0.0 
none 
none 
  VARIABLE   
DESCRIPTION
SETID 
part set ID.  See Remarks 3 and 4. 
XP 
𝑥-position  of  a  point  belonging  to  the  plane  from  which  the  3D
mesh is generated (only for a 2D to 3D mapping).  See Remark 5.
VARIABLE   
DESCRIPTION
YP 
ZP 
VECID 
ANGLE 
𝑦-position  of  a  point  belonging  to  the  plane  from  which  the  3D
mesh is generated (only for a 2D to 3D mapping).  See Remark 5. 
𝑧-position  of  a  point  belonging  to  the  plane  from  which  the  3D
mesh is generated (only for a 2D to 3D mapping).  See Remark 5. 
ID  of  the  rotation  axis  (symmetric  axis  for  a  2D  to  3D  mapping)
defined by *DEFINE_VECTOR.  See Remark 5. 
Angle of rotation around an axis defined by *DEFINE_VECTOR. 
See Remark 5. 
NELANGL 
Number  of  elements  to  create  in  the  azimuthal  direction  for
ANGLE (only for a 2D to 3D mapping).  See Remark 5. 
Remarks: 
part ids 
nodal velocities 
nodal coordinates (initial and last steps) 
nodal temperatures (if *CONTROL_THERMAL_SOLVER is used) 
1.  The Mapping File as Output.  In the absence of a *INITIAL_LAG_MAPPING 
card, adding a “lagmap=” argument to the command line will cause LS-DYNA 
to  write  a  mapping  file.    This  file  contains  the  following  nodal  and  element 
data: 
• 
• 
• 
• 
• 
• 
• 
• 
• 
• 
• 
• 
• 
element connectivities 
volume fractions 
internal energies 
relative volumes 
element centers 
bulk viscosities 
plastic strains 
densities 
stresses 
2.  The  Mapping  File  as  Input.    If  the  keyword  INITIAL_LAG_MAPPING  is  in 
the input deck and the “lagmap=” argument is in the command line, then La-
grangian data is read from the mapping file defined by “lagmap=” to initialize 
the run. 
3.  Part Sets (Write).  The part set, SETID, defines which parts are involved in the 
mapping.  The WRITE option can be used to write data in the mapping file for 
ONLY  the  parts  specified  by  the  set.    If  the  keyword  INITIAL_LAG_MAP-
PING_WRITE is not included in the input deck then ALL Lagrangian parts are 
written in the mapping file during the last cycle.  Similarly, for reading  
4.  Part Sets (Read).  The mapping initializes the data for every node and element 
defined  by  SETID  within  the  domain  swept  by  the  2D  mesh  or  the  region  ini-
tially  occupied  by  the  previous  3D  mesh.    For  nodes  and  elements  outside  of 
SETID it has no effect. 
5.  Embedding.    The  first  point  in  the  definition  of  the  rotation  axis  VECID 
specifies the origin location for the previous run in the current 3D  space.  The 
2D  to  3D  mapping  depends  on  whether  or  not  a  3D  mesh  has  already  been 
defined.  The 3D to 3D mapping needs a pre-existing mesh. 
a)  No Mesh Case for a 2D to 3D mapping.  If there is no 3D mesh (no solid and 
shell  with  parts  in  SETID),  the  point  (XP, YP, ZP)  together  with  the  sym-
metry  axis  (VECID)  are  used  to  generate  a  mesh.    The  point  defines  the 
plane in which the 2D is embedded.  The 3D mesh is generated by rotating 
the 2D mesh around the axis.  The point (XP, YP, ZP) must not be on the 
symmetry axis.  ANGLE defines the angle of rotation in degrees.  The ro-
tation is counterclockwise when viewed from the axis head.  NELANGL is 
the number of elements to generate in the azimuthal direction. 
b)  Pre-existing Mesh Case for a 2D to 3D mapping.  If there is a 3D mesh (solids 
or  shells  with  parts  in  SETID),  the  nodes  should  be  within  the  domain 
swept  by  the  initial  positions  of  the  2D  mesh.    Then,  the  nodes  are 
mapped to new locations based on the last mesh positions of the previous 
run.   
c)  Pre-existing Mesh Case for a 3D to 3D mapping.  If there is a 3D mesh (solids 
or shells with parts in SETID), the nodes should be in the region initially 
occupied by the previous 3D mesh.  Then, the nodes are mapped to new 
locations based on the last mesh positions of the previous run.  VECID is 
an  axis  of  rotation  of  the  pre-existing  mesh  if  ANGLE  is  defined.    If  this 
latter is not defined, the first point in VECID is still the previous origin lo-
cation and it can be used to translate the pre-existing mesh
*INITIAL 
Purpose:  Define initial momentum to be deposited in solid elements.  This option is to 
crudely simulate an impulsive type of loading. 
Card 
1 
Variable 
EID 
2 
MX 
Type 
I 
F 
Default 
none 
0. 
3 
MY 
F 
0. 
4 
5 
6 
7 
8 
MZ 
DEPT 
F 
0. 
F 
0, 
  VARIABLE   
DESCRIPTION
EID 
MX 
MY 
MZ 
Element ID 
Initial 𝑥-momentum 
Initial 𝑦-momentum 
Initial 𝑧-momentum 
DEPT 
Deposition time
The available options include: 
<BLANK> 
SET 
*INITIAL_PWP_DEPTH 
Purpose:    Initialize  pore  water  pressure  in  solid  elements  where  a  non-hydrostatic 
profile is required. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID/PSID 
LC 
Type 
I 
I 
Default 
none 
none 
  VARIABLE   
DESCRIPTION
Part ID or Part Set ID for the_SET option 
Curve of pore water pressure head (length units) vs 𝑧-coordinate 
PID 
LC 
Remarks: 
This  feature  overrides  the  automatically  calculated  hydrostatic  pressure  profile.    The 
points  in  the  curve  must  be  ordered  with  the  most  negative  z-coordinate  first  –  this 
order looks “upside-down” on the page.  
If  a  part  has  pore  fluid  but  no  *INITIAL_PWP_DEPTH  is  defined,  the  default  initial 
pressure profile is hydrostatic.
The available options include: 
<BLANK> 
SET 
*INITIAL 
Purpose:    Initialize  strain  tensor  for  shell  element.    This  option  is  primarily  for  multi-
stage metal forming operations where the accumulated strain is of interest. 
These strain tensors are defined at the inner and outer integration points and are used 
for post-processing only.  There is no interpolation with this option and the strains are 
defined in the global Cartesian coordinate system.  The *DATABASE_EXTENT_BINA-
RY flag STRFLG must be set to unity for this option to work.  When OPTION is blank, 
users  have  the  option  to  define  strains  at  all  integration  points  by  providing  nonzero 
NPLANE,  NTHICK  and  setting  INTOUT  flag  of  *DATABASE_EXTENT_BINARY  to 
either “STRAIN” or “ALL”. 
Card Sets.  Define as many shell elements in this section as desired, one set of cards per 
element.  The input is assumed to terminate when a new keyword is detected. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EID 
NPLANE 
NTHICK 
Type 
I 
I 
I 
Default 
none 
none 
none 
When  NPLANE  and  NTHICK  are  defined,  include  NPLANE ×  NTHICK  cards  below.  
For each through thickness point define NPLANE points.  NPLANE should be either 1 
or 4 corresponding to either 1 or 4 Gauss integration points.  If four integration points 
are specified, they should be ordered such that their in plane parametric coordinates are 
at: 
√3
⎜⎛−
⎝
, −
√3
⎟⎞ ,
3 ⎠
⎜⎛√3
⎝
, −
√3
⎟⎞ ,
3 ⎠
⎜⎛√3
⎝
,
√3
⎟⎞ ,
3 ⎠
⎜⎛−
⎝
√3
,
√3
⎟⎞ 
3 ⎠
respectively.
Strain Cards.  When NPLANE and NTHICK are not defined or when the SET option is 
used, define two cards below, one for the inner integration point and the other for the 
outer integration point, respectively.  
  Card 2 
1 
2 
3 
4 
5 
6 
Variable 
EPSxx 
EPSyy 
EPSzz 
EPSxy 
EPSyz 
EPSzx 
Type 
F 
F 
F 
Default 
none 
none 
none 
F 
F 
F 
0 
8 
7 
T 
F 
0. 
  VARIABLE   
DESCRIPTION
EID 
Element ID or shell element set ID when the SET option is used. 
NPLANE 
NTHICK 
EPSij 
T 
Number  of  in-plane  integration  points  being  output  (not  read
when the SET option is used).  
Number  of  integration  points  through  the  thickness  (not  read
when the SET option is used). 
Define  the  ij  strain  component.    The  strains  are  defined  in  the
GLOBAL Cartesian system. 
Parametric  coordinate  of  through  thickness  integration  point
between -1 and 1 inclusive.
The availables options include: 
<BLANK> 
SET 
*INITIAL 
Purpose:  Initialize  strain tensor at element  center.  This option can be  used  for multi-
stage metal forming operations where the accumulated strain is of interest. 
These strain tensors are defined at the element center and are used for post-processing 
only.  The strains are  defined in the global  Cartesian coordinate system.  The *DATA-
BASE_EXTENT_BINARY  flag  STRFLG  must  be  set  to  unity  for  this  option  to  work.  
This  capability  is  not  available  for  the  cohesive  element  since  it  is  based  on 
displacements, not strains. 
Card Sets.  Define as many solid elements in this section as desired: one pair of cards per 
element.  The input is assumed to terminate when a new keyword is detected. 
Element ID Cards. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EID 
Type 
I 
Default 
none 
Strain Cards. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EPSxx 
EPSyy 
EPSzz 
EPSxy 
EPSyz 
EPSzx 
Type 
F 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
EID 
EPSij 
Element ID or solid element set ID when the SET option is used. 
Define  the  ij  strain  component.    The  strains  are  defined  in  the
GLOBAL cartesian system.
*INITIAL_STRAIN_TSHELL 
Purpose:  Initialize the strain tensors for thick shell elements.. 
Strain  tensors  are  defined  at  the  inner  and  outer  integration  points  and  are  used  for 
post-processing  only.    Strain  tensors  are  defined  in  the  global  Cartesian  coordinate 
system.  The STRFLG flag on *DATABASE_EXTENT_BINARY must be set to unity for 
this option to work.  Initialize as many elements as needed. 
Card Sets.  For each element, include a set of cards 1, 2, and 3, where card 2 is for the 
inner layer and card 3 is for the outer layer.  The input is assumed to terminate when a 
new keyword is detected 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EID 
Type 
I 
Default 
none 
Strain Cards.  Card 2 is the strain at the inner layer.  Card 3 is the strain at the outer 
layer. 
Cards 2, 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EPSxx 
EPSyy 
EPSzz 
EPSxy 
EPSyz 
EPSzx 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
. 
  VARIABLE   
DESCRIPTION
EID 
EPSij 
Element ID. 
Define  the  ij  strain  component.    The  strains  are  defined  in  the
GLOBAL Cartesian system.
*INITIAL 
Purpose:    Initialize  stresses,  plastic  strains  and  history  variables  for  Hughes-Liu  beam 
elements,  or  the  axial  force,  moment  resultants  and  history  variables  for  Belytschko-
Schwer beam elements. 
Card Sets.  Define as many beams in this section as desired.  Each set consists of one 
Card  1  and  several  additional  cards  depending  on  variables  NPTS,  LARGE,  NHISV, 
and NAXES.  The input terminates when a new keyword (“*”) card is detected. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EID 
RULE 
NPTS 
LOCAL 
LARGE 
NHISV 
NAXES 
Type 
I 
I 
I 
Default 
none 
none 
none 
I 
0 
I 
0 
I 
0 
I 
0 
Belytschko-Schwer Card for LARGE = 0.  Additional card for the Belytschko-Schwer 
beam. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
F11 
T11 
M12 
M13 
M22 
M23 
PARM 
Type 
F 
F 
F 
F 
F 
F 
F 
Belytschko-Schwer  Cards  for  LARGE = 1.    Additional  cards  for  the  Belytschko-
Schwer beam.  Include as many cards as necessary to collect NHISV  history 
variables. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
F11 
Type 
F 
T11 
F 
M12 
M13 
M22 
F 
F
*INITIAL_STRESS_BEAM 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
M23 
PARM 
HISV1 
HISV2 
HISV3 
Type 
F 
F 
F 
F 
F 
Hughes-Liu  Cards  for  LARGE = 0.    Additional  cards  for  the  Hughes-Liu  beam. 
Include NPTS additional cards, one per integration point. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SIG11 
SIG22 
SIG33 
SIG12 
SIG23 
SIG31 
EPS 
Type 
F 
F 
F 
F 
F 
F 
F 
Hughes-Liu  Cards  for  LARGE = 1.    Additional  cards  for  the  Hughes-Liu  beam. 
Include NPTS additional card sets, one per integration point.  Include as many cards in 
one card set as necessary to collect NHISV  history variables. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
SIG11 
SIG22 
SIG33 
SIG12 
SIG23 
Type 
F 
F 
F 
F 
F 
. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
SIG31 
Type 
F 
EPS 
F 
HISV1 
HISV2 
HISV3 
F 
F
Optional Local Axes Cards for NAXES = 12.  Additional cards for definition of local 
axes values.  These 12 values are internally used by LS-DYNA for the mapping between 
local  beam  element  system  and  global  coordinate  system.    They  are  automatically 
written  to  the  dynain  file  if  *INTERFACE_SPRINGBACK_LSDYNA  or  *CONTROL_-
STAGED_CONSTRUCTION is used.  
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
AX1 
Type 
F 
AX2 
F 
AX3 
F 
AX4 
F 
AX5 
F 
. 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
AX6 
Type 
F 
AX7 
F 
AX8 
F 
AX9 
F 
AX10 
F 
. 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
AX11 
AX12 
Type 
F 
F 
  VARIABLE   
DESCRIPTION
EID 
Element ID 
RULE 
Integration rule type number: 
EQ.1.0: 1 × 1 Gauss quadrature, 
EQ.2.0: 2 × 2 Gauss quadrature (default beam), 
EQ.3.0: 3 × 3 Gauss quadrature, 
EQ.4.0: 3 × 3 Lobatto quadrature, 
EQ.5.0: 4 × 4 Gauss quadrature. 
NPTS 
Number  of  integration  points. 
resultant beam element, NPTS = 1. 
  For  the  Belytschko-Schwer
*INITIAL_STRESS_BEAM 
DESCRIPTION
LOCAL 
Coordinate system for stresses: 
EQ.0: Stress  components  are  defined  in  the  global  coordinate
system. 
EQ.1: Stress components are defined in the local beam system.
In the local system components SIG22, SIG33, and SIG23
are set to 0.0. 
LARGE 
Format size: 
EQ.0:  off, 
EQ.1:  on.  Each field is twice as long for higher precision. 
NHISV 
Number  of  additional  history  variables.    Only  available  for
LARGE = 1. 
NAXES 
Number of variables giving beam local axes (0 or 12) 
F11 
T11 
M12 
M13 
M22 
M23 
Axial force resultant along local beam axis 1 
Torsional moment resultant about local beam axis 1 
Moment resultant at node 1 about local beam axis 2 
Moment resultant at node 1 about local beam axis 3 
Moment resultant at node 2 about local beam axis 2 
Moment resultant at node 2 about local beam axis 3 
PARM 
Generally not used. 
SIGij 
EPS 
Define the ij stress component 
Effective plastic strain 
HISVn 
Define the nth history variable 
AXn 
The nth local axes value
Available options include: 
<BLANK> 
SET 
*INITIAL 
Purpose:  Initialize solid element stresses where stress is a function of depth. 
  Card 1 
1 
2 
3 
4 
Variable 
PID/PSID 
RO_G 
ZDATUM 
KFACT 
Type 
I 
F 
F 
F 
5 
LC 
I 
6 
7 
8 
LCH 
LCK0 
I 
I 
Default 
none 
none 
none 
0.0 
none 
none 
none 
  VARIABLE   
DESCRIPTION
PID/PSID 
Part ID or Part Set ID for the SET option 
RO_G 
Stress per unit elevation above datum, which is usually 
𝜌𝑔 = density × gravity.
ZDATUM 
𝑧-coordinate of datum 
KFACT 
𝑥 and 𝑦-stresses = KFACT × 𝑧-stress 
Optional  curve  of  stress  vs  z-coordinate  (ZDATUM  is  ignored 
with this option) 
Optional curve of horizontal stress versus z-coordinate (KFACT is 
ignored with this option) 
Optional  curve  of  K0  (ratio  of  horizontal_stress/vertical_stress) 
versus  𝑧-coordinate.    KFACT  and  LCH  are  ignored  with  this 
option.    The  𝑥-axis  of  the  curve  is  the  𝑧-coordinate,  the  𝑦-axis  is 
K0. 
LC 
LCH 
LVK0 
Remarks: 
With this keyword stress is calculated according to,
σz = RO G × (Zelement − ZDATUM). 
To generate compressive stresses, the datum should be above the highest element.  For 
instance, this is usually at the surface of the soil in geotechnics simulations.  If the curve 
is present, it overrides RO_G and ZDATUM.  Note that the points in the curve should 
be ordered with most negative 𝑧-coordinate first. 
First, select how the vertical stress as a function of 𝑧-coordinate will be defined (either 
RO_G  and  ZDATUM,  or  LC).    Next,  select  how  the  horizontal  stress  will  be  defined 
(either a constant factor KFACT times the vertical stress; or a factor that varies with 𝑧-
coordinate  times  the  vertical  stress  using  LCK0;  or  a  curve  of  horizontal  stress  versus 
depth LCH). 
If pore water is present, the stresses input here are effective (soil skeleton stresses only).  
The  pore  water  pressures  will  automatically  be  initialized  to  hydrostatic,  or  by  *INI-
TIAL_PWP_DEPTH or *BOUNDARY_PWP_TABLE if those cards are present. 
For a 2D problem (axisymmetric or plane strain), replace 𝑧 in above documentation with 
𝑦.
*INITIAL 
Purpose:  Initialize the stress in solid elements that are included in a section definition 
(*DATABASE_CROSS_SECTION_option) to create a preload.  The stress component in 
the direction normal to the cross-section plane is prescribed according to a curve.  This 
option  works  with  a  subset  of  materials  that  are  incrementally  updated  including  the 
elastic, viscoelastic, and elastoplastic materials.  Rubbers, foams, and materials that are 
combined  with  equations-of-state  cannot  be  initialized  by  this  approach,  except  as 
noted in Remark #3. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ISSID 
CSID 
LCID 
PSID 
VID 
IZSHEAR 
Type 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
I 
0 
  VARIABLE   
DESCRIPTION
ISSID 
CSID 
LCID 
PSID 
VID 
Section stress initialization ID. 
Cross-section ID.  See *DATABASE_CROSS_SECTION. 
Load  curve  ID  defining  preload  stress  versus  time.    When  the
load curve ends or goes to zero, the initialization is assumed to be
completed.  See Remark 2. 
Part set ID. 
Vector ID defining the direction normal to the cross section.  This
vector must be defined if *DATABASE_CROSS_SECTION_SET is 
used  to  define  the  cross  section.    If  the  cross  section  is  defined
using the PLANE option, the normal used in the definition of the
plane is used if VID is left undefined. 
IZSHEAR 
Shear stress flag:  
EQ.0: Shear  stresses  are  prescribed  as  zero  during  the  time
the curve is acting to prescribe normal stress. 
EQ.1:    Shear  stresses  are  allowed  to  develop  during  the  time
the curve is acting to prescribe normal stress.
*INITIAL_STRESS_SECTION 
1.  To  achieve  convergence  during  explicit  dynamic  relaxation,  the  application  of 
the damping options is very important.  If contact is active, contact damping is 
recommended  with  a  value  between  10-20  percent.    Additional  damping,  via 
the  option  DAMPING_PART_STIFFNESS  also  speeds  convergence  where  a 
coefficient of 0.10 is effective.    If damping is not used, convergence may not be 
possible. 
2.  When  defining  the  load  curve,  LCID,  a  ramp  starting  at  the  origin  should  be 
used to increase the stress to the desired value.  The time duration of the ramp 
should  produce  a  quasi-static  response.      When  the  end  of  the  load  curve  is 
reached, or when the value of the load decreases from its maximum value, the 
initialization stops.  If the load curve begins at the desired stress value, i.e., no 
ramp, convergence will take much longer, since the impulsive like load created 
by  the  initial  stress  can  excite  nearly  every  frequency  in  the  structural  system 
where stress is initialized. 
3.  This option currently applies only to materials that are incrementally updated.  
Hyperelastic  materials  and  materials  that  require  an  equation-of-state  are  not 
currently supported.  However, materials 57, 73, and 83 can be initialized with 
this approach. 
4.  Solid elements types 1, 2, 3, 4, 9, 10, 13, 15, 16, 17, and 18 are supported.  ALE 
elements are not supported.
Available options include: 
<BLANK> 
SET 
*INITIAL 
Purpose:    Initialize  stresses,  history  variables,  and  the  effective  plastic  strain  for  shell 
elements.    Materials  that  do  not  use  an  incremental  formulation  for  the  stress  update 
may not be initializable with this card. 
Card  Sets  per  Element.    Define  as  many  shell  elements  or  shell  element  sets  in  this 
section as desired.  The input is assumed to terminate when a new keyword (“*”) card is 
detected. 
Element Card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EID/SID 
NPLANE 
NTHICK 
NHISV 
NTENSR 
LARGE 
NTHINT 
NTHHSV 
Type 
I 
I 
I 
Default 
none 
none 
none 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
Ordering of Integration Points. 
For each through thickness point define NPLANE points.  NPLANE should be either 1 
or 4 corresponding to either 1 or 4 Gauss integration points.  If four integration points 
are specified, they should be ordered such that their in plane parametric coordinates are 
at: 
√3
⎜⎛−
⎝
, −
√3
⎟⎞ ,
3 ⎠
⎜⎛√3
⎝
, −
√3
⎟⎞ ,
3 ⎠
⎜⎛√3
⎝
,
√3
⎟⎞ ,
3 ⎠
⎜⎛−
⎝
√3
,
√3
⎟⎞ , 
3 ⎠
respectively.    It  is  not  necessary  for  the  location  of  the  through  thickness  integration 
points  to  match  those  used  in  the  elements  which  are  initialized.    The  data  will  be 
interpolated by LS DYNA. 
Solid Mechanics Data Card for LARGE = 0. 
The following set of cards: “Stress Card” through “Tensor Cards.”  Should be included 
NPLANE × NTHICK times (one set for each integration point).
Stress Card.  Additional Card for LARGE = 0. 
  Card 2 
Variable 
Type 
1 
T 
F 
2 
3 
4 
5 
6 
7 
8 
SIGXX 
SIGYY 
SIGZZ 
SIGXY 
SIGYZ 
SIGZX 
EPS 
F 
F 
F 
F 
F 
F 
F 
History Variable Cards.  Additional Cards for LARGE = 0.  Include as many cards as 
necessary to collect NHISV  history variables. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
HISV1 
HISV2 
HISV3 
HISV4 
HISV5 
HISV6 
HISV7 
HISV8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Tensor Cards.  Additional card for LARGE = 0.  Include as many cards as necessary to 
collect NTENSR  entries.  Tensor cards contain only 6 entries per card. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TENXX 
TENYY 
TENZZ 
TENXY 
TENYZ 
TENZX 
Type 
F 
F 
F 
F 
F 
F 
Solid Mechanics Data Card for LARGE = 1. 
The  following  set  of  cards:  “Stress  Card  1”  through  “Tensor  Cards.”    Should  be 
included NPLANE × NTHICK times (one set for each integration point). 
Stress Card 1.  Additional Card for LARGE = 1. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
Type 
T 
F 
SIGXX 
SIGYY 
SIGZZ 
SIGXY 
F 
F 
F
Stress Card 2.  Additional Card for LARGE = 1. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
SIGYZ 
SIGZX 
Type 
F 
F 
EPS 
F 
History Variable Cards.  Additional Cards for LARGE = 1.  Include as many cards as 
necessary to collect NHISV  history variables. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
HISV1 
HISV2 
HISV3 
HISV4 
HISV5 
Type 
F 
F 
F 
F 
F 
Tensor Cards.  Include as many pairs of Cards 5 and 6 as necessary to collect NTENSR 
entries.    Note  that  Cards  5  and  6  must  allows  appear  as  pairs,  and  that  Card  6  may 
include at most one value, as indicated below. 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
TENXX 
TENYY 
TENZZ 
TENXY 
TENYZ 
Type 
F 
F 
F 
F 
F 
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
TENZX 
Type 
F 
Thermal Data Cards for LARGE = 1. 
For each element, thermal data cards come after the entire set of mechanical data cards.  
For each of the NTHINT thermal integration points, include the following set of cards.
Thermal  Time  History  Cards.    Additional  cards  for  LARGE = 1.    Include  as  many 
cards  as  needed  to  collect  all  the  of  NTHHSV  time  history  variables  per  thermal 
integration point. 
  Card 7 
1 
2 
3 
4 
5 
Variable 
THHSV1 
THHSV2 
THHSV3 
THHSV4 
THHSV5 
Type 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
EID/SID 
Element ID or shell set ID, see *SET_SHELL_… 
NPLANE 
Number of in plane integration points being output. 
NTHICK 
Number of integration points through the thickness. 
NHISV 
Number of additional history variables. 
NTENSR 
Number  of  components  of  tensor  data  taken  from  the  element
history variables stored. 
LARGE 
Format size.  See cards above. 
EQ.0:  off 
EQ.1:  on 
T 
SIGij 
Parametric  coordinate  of  through  thickness  integration  point
between -1 and 1 inclusive. 
Define  the  ij  stress  component.    The  stresses  are  defined  in  the
GLOBAL cartesian system. 
EPS 
Effective plastic strain. 
HISVn 
TENij 
Define the nth history variable. 
Define  the  ijth  component  of  the  tensor  taken  from  the  history
variables.  The tensor is defined in the GLOBAL Cartesian system.
Define enough lines to provide a total of NTENSOR components,
stored six components per line.  This applies to material 190 only.
NTHINT 
Number of thermal integration points.
VARIABLE   
NTHHSV 
DESCRIPTION
Number  of  thermal  history  variables  per  thermal  integration
point. 
THHSVn 
nth history variable at the thermal integration point.
*INITIAL_STRESS_SOLID_{OPTION} 
Available options include: 
<BLANK> 
SET 
Purpose:  Initialize stresses and plastic strains for solid elements.  This command is not 
applicable to hyperelastic materials or any material model based on a Total Lagrangian 
formulation.    Furthermore,  for  *MAT_014  and  any  material  that  requires  an  equation-
of-state  (*EOS),  the  specified  initial  stresses  are  adjusted  to  be  in  accordance  with  the 
initial pressure calculated from the equation of state. 
Card Sets per Element.  For this keyword, each data card set consists of an element or 
element set card and all of its corresponding data cards, both thermal and mechanical.  
For LARGE = 1, this can involve several (even tens of) cards per set.  Include cards for 
as  many  solid  elements  or  solid  element  sets  as  desired.    The  input  is  assumed  to 
terminate when a new keyword (“*”) card is detected. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EID/SID 
NINT 
NHISV 
LARGE 
IVEFLG 
IALEGP 
NTHINT 
NTHHSV 
Type 
I 
I 
Default 
none 
none 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
Ordering of Integration Points. 
NINT  may  be  1,  8,  or  14  for  hexahedral  solid  elements,  depending  on  the  element 
formulation.    If  eight  Gauss  integration  points  are  specified,  they  should  be  ordered 
such that their parametric coordinates are located at: 
, −
, −
, −
, −
√3
√3
√3
⎜⎛−
⎝
⎜⎛√3
⎝
√3
⎟⎞ ,
3 ⎠
√3
⎟⎞ ,
3 ⎠
respectively.    If  eight  points  are  defined  for  1  point  LS-DYNA  solid  elements,  the 
average value will be taken. 
√3
⎟⎞ ,
3 ⎠
√3
⎟⎞ ,
3 ⎠
⎜⎛√3
⎝
⎜⎛√3
⎝
√3
⎟⎞ , 
3 ⎠
√3
⎟⎞ ,
3 ⎠
√3
⎟⎞ ,
3 ⎠
⎜⎛√3
⎝
√3
3 ⎠
⎜⎛−
⎝
⎜⎛−
⎝
⎜⎛−
⎝
√3
√3
√3
√3
√3
√3
√3
√3
√3
⎟⎞,  
, −
, −
, −
, −
,
,
,
,
,
,
,
,
NINT  may  be  1,  4,  or  5  for  tetrahedral  solid  elements,  depending  on  the  element 
formulation and NIPTETS in *CONTROL_SOLID.  NINT may be 1 or 2 for pentahedral 
solid elements, depending on the element formulation. 
Solid Mechanics Data Card for LARGE = 0. 
Stress  Card.    Additional  Card  for  LARGE = 0.    This  card  should  be  included  NINT 
times (one for each integration point). 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SIGXX 
SIGYY 
SIGZZ 
SIGXY 
SIGYZ 
SIGZX 
EPS 
Type 
F 
F 
F 
F 
F 
F 
F 
Mechanical Data Cards for LARGE = 1. 
The following set of cards “Stress Card 1” through “Additional History Cards.”  Should 
be included NINT times (one set for each integration point). 
Stress Card 1.  Additional cards for LARGE = 1. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
SIGXX 
SIGYY 
SIGZZ 
SIGXY 
SIGYZ 
Type 
F 
F 
F 
F 
F 
Stress Card 2.  Additional cards for LARGE = 1. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
SIGZX 
Type 
F 
EPS 
F 
HISV1 
HISV2 
HISV3 
F 
F
Additional  History  Cards.    Additional  cards  for  LARGE = 1.    If  NHISV > 3  define  as 
many additional cards as necessary.  NOTE: the value of IVEFLG  can affect 
the number of history variables on these cards. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
HISV1 
HISV2 
HISV3 
HISV4 
HISV5 
Type 
F 
F 
F 
F 
F 
Thermal Data Cards for LARGE = 1. 
For each element, thermal data cards come after the entire set of mechanical data cards.  
For each of the NTHINT thermal integration points, include the following set of cards. 
Thermal  Time  History  Cards.    Additional  cards  for  LARGE = 1.    Include  as  many 
cards  as  needed  to  capture  all  the  of  NTHHSV  time  history  variables  per  thermal 
integration point. 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
THHSV1 
THHSV2 
THHSV3 
THHSV4 
THHSV5 
Type 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
EID/SID 
Element ID or solid set ID, see *SET_SOLID_... 
NINT 
NHISV 
LARGE 
Number  of  integration  points  (should  correspond  to  the  solid
element formulation). 
Number  of  additional  history  variables,  which  is  typically  equal
to the number of history variables stored at the integration point 
+ IVEFLG. 
Format  size,  if  zero,  NHISV  must  also  be  set  to  zero  (this  is  the
format used by LS-DYNA versions 970 and earlier) and, if  set to
1, a larger format is used and NHISV is used.
VARIABLE   
DESCRIPTION
IVEFLG 
Initial Volume/energy flag (only used in large format) 
EQ.0: last history variable is used as normal, 
EQ.1: last  history  variable  is  used  as  the  initial  volume  of  the
element.    One  additional  history  variable  is  required  if
IVFLG = 1 
EQ.2: last  two  history  variables  are  used  to  define  the  initial
volume  and  the  internal  energy  per  unit  initial  volume.
Two  additional  history  variables  must  be  allocated,  see
NHISV above, if IVFLG = 2.  If the initial volume is set to 
zero, the actual element volume is used. 
The ALE multi-material group (AMMG) ID; only if the element is
of ALE multi-material formulation (ELEFORM = 11).  In this case, 
each AMMG has its own sets of stress and history variables so we
must  specify  to  which  AMMG  the  stress  data  are  assigned.    For
mixed elements, multiple cards are needed to complete the stress
initialization  in  this  element  as  each  AMMG  needs  to  have  its
own set of stress data. 
EQ.0: Assuming  the  element  is  fully  filled  by  the  AMMG  that 
the element part belongs to.  Please refer to *ALE_MUL-
TI-MATERIAL_GROUP card.  
EQ.n: Assigning the stress to nth AMMG in that element. 
Define  the  ijth  stress  component.    Stresses  are  defined  in  the
GLOBAL Cartesian system. 
Effective plastic strain 
Define (𝑁𝐻𝑆𝑉 + 𝐼𝑉𝐸𝐹𝐿𝐺) history variables. 
IALEGP 
SIGij 
EPS 
HISVi 
NTHINT 
Number of thermal integration points 
NTHHSV 
Number  of  thermal  history  variables  per  thermal  integration
point 
THHSVn 
nth thermal time history variable 
Remarks: 
1.  The  elastic  material  model  for  cohesive  elements  is  a  total  Lagrangian 
formulation, and the initial stress will therefore be ignored for it.
*INITIAL_STRESS_SPH 
Purpose:  Initialize stresses and plastic strains for SPH elements.  This command is not 
applicable to hyperelastic materials or any material model based on a Total Lagrangian 
formulation.  For *MAT_005, *MAT_014, and any material that requires an equation-of-
state (*EOS), the initialized stresses are deviatoric stresses, not total stresses. 
Element Cards.  Define as many SPH elements in this section as desired.  The input is 
assumed to terminate when a new keyword is detected.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EID 
SIGXX 
SIGYY 
SIGZZ 
SIGXY 
SIGYZ 
SIGZX 
EPS 
Type 
I 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
EID 
SIGij 
SPH particle ID 
Define  the  ijth  stress  component.    Stresses  are  defined  in  the
GLOBAL Cartesian system. 
EPS 
Effective plastic strain.
*INITIAL 
Purpose:  Initialize stresses and plastic strains for thick shell elements. 
Card Sets per Element.  Define as many thick shell elements in this section as desired.  
The input is assumed to terminate when a new keyword is detected. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EID 
NPLANE 
NTHICK 
NHISV 
LARGE 
Type 
I 
I 
I 
Default 
none 
none 
none 
I 
0 
I 
0 
Ordering of Integration Points. 
For each through thickness point define NPLANE points.  NPLANE should be either 1 
or 4 corresponding to either 1 or 4 Gauss integration points.  If four integration points 
are specified, they should be ordered such that their in plane parametric coordinates are 
at: 
√3
⎜⎛−
⎝
, −
√3
⎟⎞ ,
3 ⎠
⎜⎛√3
⎝
, −
√3
⎟⎞ ,
3 ⎠
⎜⎛√3
⎝
,
√3
⎟⎞ ,
3 ⎠
⎜⎛−
⎝
√3
,
√3
⎟⎞ 
3 ⎠
respectively.    It  is  not  necessary  for  the  location  of  the  through  thickness  integration 
points  to  match  those  used  in  the  elements  which  are  initialized.    The  data  will  be 
interpolated by LS DYNA. 
Data Card for LARGE = 0. 
The  following  set  of  cards  “Stress  Card”  and  “History  Cards.”    Should  be  included 
NPLANE × NTHICK times (one set for each integration point).
Stress Card.  Additional card for LARGE = 0. 
  Card 2 
Variable 
Type 
1 
T 
F 
2 
3 
4 
5 
6 
7 
8 
SIGXX 
SIGYY 
SIGZZ 
SIGXY 
SIGYZ 
SIGZX 
EPS 
F 
F 
F 
F 
F 
F 
F 
History  Cards.    Additional  Card  for  LARGE = 0.    Include  as  many  History  Cards  as 
needed to define all NHIST history variables. 
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
HISV1 
HSIV2 
HSIV3 
HSIV4 
HSIV5 
HSIV6 
HSIV7 
HSIV8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Data Card for LARGE = 1. 
The  following  set  of  cards  “Stress  Cards”  and  “History  Cards.”    Should  be  included 
NPLANE × NTHICK times (one set for each integration point). 
Stress Card 1.  Additional card for LARGE = 1.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
Type 
T 
F 
SIGXX 
SIGYY 
SIGZZ 
SIGXY 
F 
F 
F 
F 
Stress Card 2.  Additional card for LARGE = 3. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
SIGYZ 
SIGZX 
Type 
F 
F 
EPS
History  Cards.    Additional  Card  for  LARGE = 1.    Include  as  many  History  Cards  as 
needed to define all NHIST history variables. 
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
HISV1 
HISV2 
HISV3 
HISV4 
HISV5 
Type 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
EID 
Element ID 
NPLANE 
Number of in plane integration points. 
NTHICK 
Number of integration points through the thickness. 
T 
Parametric  coordinate  of  through  thickness  integration  point
between -1 and 1 inclusive. 
NHISV 
Number of additional history variables. 
LARGE 
Format size.  See keywords above. 
EQ.0:  off 
EQ.1:  on 
SIGij 
Define  the  ij  stress  component.    The  stresses  are  defined  in  the
GLOBAL Cartesian system. 
EPS 
Effective plastic strain
Available options include: 
NODE 
SET 
*INITIAL_TEMPERATURE 
Purpose:  Define initial nodal point temperatures using nodal set ID’s or node numbers.  
These  initial  temperatures  are  used  in  a  thermal  only  analysis  or  a  coupled 
thermal/structural analysis.  See also *CONTROL_THERMAL_SOLVER, *CONTROL_-
THERMAL_TIMESTEP, and CONTROL_THERMAL_NONLINEAR. 
For thermal loading in a structural only analysis, see *LOAD_THERMAL_OPTION. 
Node/Node set Cards.  Include one card for each node or node set.  This input ends at 
the next keyword (“*”) keyword. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  NSID/NID 
TEMP 
LOC 
Type 
I 
I 
Default 
none 
0. 
I 
0 
Remark 
1 
  VARIABLE   
DESCRIPTION
NSID/NID 
Nodal set ID or nodal point ID, see also *SET_NODES: 
EQ.0: all nodes are included (set option only). 
TEMP 
Temperature at node or node set. 
LOC 
For  a  thick  thermal  shell,  the  temperature  will  be  applied  to  the
surface  identified  by  LOC,  See  parameter,  THSHEL,  on  the 
*CONTROL_SHELL keyword. 
EQ.-1: lower surface of thermal shell element 
EQ.0:  middle surface of thermal shell element 
EQ.1:  upper surface of thermal shell element
*INITIAL 
1.  This  keyword  can  be  used  to  define  initial  nodal  point  temperatures  for  SPH 
particles by using nodal set ID’s or node numbers from SPH particles.
*INITIAL_VEHICLE_KINEMATICS 
Purpose:  Define initial kinematical information for a vehicle.  In its initial orientation, 
the vehicle’s yaw, pitch, and roll axes must be aligned with the global axes.  Successive 
simple rotations are taken about these body fixed axes. 
  Card 1 
1 
2 
Variable 
GRAV 
PSID 
Type 
I 
I 
3 
XO 
F 
Default 
none 
none 
0. 
4 
YO 
F 
0. 
5 
ZO 
F 
0. 
6 
XF 
F 
0. 
7 
YF 
F 
0. 
8 
ZF 
F 
0. 
  Card 2 
Variable 
1 
VX 
Type 
F 
Default 
0. 
2 
VY 
F 
0. 
3 
VZ 
F 
0. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
AAXIS 
BAXIS 
CAXIS 
I 
0 
4 
I 
0 
5 
I 
0 
6 
7 
8 
Variable 
AANG 
BANG 
CANG 
WA 
WB 
WC 
Type 
F 
Default 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0.
gravity
roll
yaw
pitch
Figure 23-3.  The vehicle pictured is to be oriented with a successive rotation
sequence  about  the  yaw,  pitch,  and  roll  axes,  respectively.    Accordingly,
AAXIS = 3,  BAXIS = 1,  and  CAXIS = 2.    The  direction  of  gravity  is  given  by
GRAV = -3. 
  VARIABLE   
DESCRIPTION
GRAV 
Gravity direction code. 
EQ.1:  Global +𝑥 direction. 
EQ.-1:  Global −𝑥 direction. 
EQ.2:  Global +𝑦 direction. 
EQ.-2:  Global −𝑦 direction. 
EQ.3:  Global +𝑧 direction. 
EQ.-3:  Global −𝑧 direction. 
Note:    this  must  be  the  same  for  all  vehicles  present  in  the
model. 
PSID 
Part set ID. 
XO 
YO 
ZO 
XF 
YF 
ZF 
VX 
𝑥-coordinate of initial position of mass center. 
𝑦-coordinate of initial position of mass center. 
𝑧-coordinate of initial position of mass center. 
𝑥-coordinate of final position of mass center. 
𝑦-coordinate of final position of mass center. 
𝑧-coordinate of final position of mass center. 
global 𝑥-component of mass center velocity.
VY 
VZ 
*INITIAL_VEHICLE_KINEMATICS 
DESCRIPTION
global 𝑦-component of mass center velocity. 
global 𝑧-component of mass center velocity. 
AAXIS 
First rotation axis code. 
EQ.1: Initially aligned with global 𝑥-axis. 
EQ.2: Initially aligned with global 𝑦-axis. 
EQ.3: Initially aligned with global 𝑧-axis. 
BAXIS 
CAXIS 
Second rotation axis code. 
Third rotation axis code. 
AANG 
Rotation angle about the first rotation axis (degrees). 
BANG 
CANG 
WA 
WB 
WC 
Rotation angle about the second rotation axis (degrees). 
Rotation angle about the third rotation axis (degrees). 
Angular  velocity  component 
(radian/second). 
Angular  velocity  component 
(radian/second). 
Angular  velocity  component 
(radian/second). 
for 
the  𝑥  body-fixed  axis 
for 
the  𝑦  body-fixed  axis 
for 
the  𝑧  body-fixed  axis
*INITIAL 
Purpose:    Define  initial  nodal  point  velocities  using  nodal  set  ID’s.    This  may  also  be 
used for sets in which some nodes have other velocities.  See NSIDEX below. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSID 
NSIDEX 
BOXID 
IRIGID 
ICID 
Type 
I 
Default 
none 
Remark 
1 
  Card 2 
Variable 
1 
VX 
Type 
F 
Default 
0. 
I 
0 
2 
VY 
F 
0. 
I 
0 
3 
VZ 
F 
0. 
I 
0 
I 
0 
4 
5 
6 
7 
8 
VXR 
VYR 
VZR 
F 
0. 
F 
0. 
F 
0. 
Exempted Node Card.  Additional card for NSIDEX > 0.  
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VXE 
VYE 
VZE 
VXRE 
VYRE 
VZRE 
Type 
F 
Default 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
  VARIABLE   
NSID 
DESCRIPTION
Nodal  set  ID,  see  *SET_NODES,  containing  nodes  for  initial 
velocity:  If NSID = 0 the initial velocity is applied to all nodes.
NSIDEX 
BOXID 
IRIGID 
ICID 
VX 
VY 
VZ 
VXR 
VYR 
VZR 
VXE 
VYE 
*INITIAL_VELOCITY 
DESCRIPTION
Nodal  set  ID,  see  *SET_NODES,  containing  nodes  that  are 
exempted from the imposed velocities and may have other initial
velocities. 
All  nodes  in  box  which  belong  to  NSID  are  initialized.    Nodes
  Exempted  nodes  are
outside  the  box  are  not  initialized. 
initialized  to  velocities  defined  by  VXE,  VYE,  and  VZE  below 
regardless of their location relative to the box. 
Option  to  overwrite  rigid  body  velocities  defined  on  *PART_IN-
ERTIA  and  *CONSTRAINED_NODAL_RIGID_BODY_INERTIA 
cards. 
GE.1:  part set ID, containing ID of parts to overwrite.  Center 
of gravity of part must lie within box BOXID.  If BOXID
is not defined then all parts defined in the set are over-
written. 
EQ.-1:  Overwrite  velocities  for  all  *PART_INERTIA's  and 
*CONSTRAINED_NODAL_RIGID_BODY_INERTIA's 
with a center of gravity within box BOXID.  If BOXID is 
not defined then all are overwritten. 
EQ.-2:  Overwrite  velocities  for  all  *PART_INERTIA's  and 
*CONSTRAINED_NODAL_RIGID_BODY_INERTIA's. 
Local coordinate system ID.  The initial velocity is specified in the
local coordinate system if ICID is greater than zero.  Furthermore,
if  ICID  is  greater  than  zero,  *INCLUDE_TRANSFORM  does  not
rotate the initial velocity values specificied by VX, VY, …, VZRE. 
Initial translational velocity in 𝑥-direction 
Initial translational velocity in 𝑦-direction 
Initial translational velocity in 𝑧-direction 
Initial rotational velocity about the 𝑥-axis 
Initial rotational velocity about the 𝑦-axis 
Initial rotational velocity about the 𝑧-axis 
Initial velocity in 𝑥-direction of exempted nodes 
Initial velocity in 𝑦-direction of exempted nodes
VARIABLE   
DESCRIPTION
Initial velocity in 𝑧-direction of exempted nodes 
Initial rotational velocity in 𝑥-direction of exempted nodes 
Initial rotational velocity in 𝑦-direction of exempted nodes 
Initial rotational velocity in 𝑧-direction of exempted nodes 
VZE 
VXRE 
VYRE 
VZRE 
Remarks: 
1.  This generation input must not be used with *INITIAL_VELOCITY_GENERA-
TION keyword.  
2. 
If a node is initialized on more than one input card set, then the last set input 
will determine its velocity.  However, if the nodal velocity is also specified on a 
*INITIAL_VELOCITY_NODE  card,  then  the velocity  specification  on  this  card 
will be used. 
3.  Unless  the  option  IRIGID  is  specified  rigid  bodies,  initial  velocities  given  in 
*PART_INERTIA will overwrite generated initial velocities.   The IRIGID option 
will  cause  the  rigid  body  velocities  specified  on  the  *PART_INERTIA  input  to 
be overwritten.  To directly specify the motion of a rigid body without using the 
keyword,  *PART_INERTIA,  which  also  requires  the  definition  of  the  mass 
properties, use the keyword option, *INITIAL_VELOCITY_RIGID_BODY. 
4.  Nodes  which  belong  to  rigid  bodies  must  have  motion  consistent  with  the 
translational  and  rotational  velocity  of  the  center  of  gravity  (c.g.)  of  the  rigid 
body.    During  initialization  the  rigid  body  translational  and  rotational  rigid 
body momentum's are computed based on the prescribed nodal velocity field.  
From  this  rigid  body  momentum,  the  translational  and  rotational  velocities  of 
the nodal points are computed and reset to the new values.  These new values 
may or may not be the same as the values  prescribed for the nodes that make 
up the rigid body.  Sometimes this occurs in single precision due to numerical 
round-off.  If a problem like this occurs specify the velocity using the keyword: 
*INITIAL_VELOCITY_RIGID_BODY. 
5.  Mid-side  nodes  generated  by  *ELEMENT_SOLID_TET4TO10  will  not  be 
initialized since the node numbers are not known a priori to the user.  Instead 
use *INITIAL_VELOCITY_GENERATION if you intend to initialize the veloci-
ties of the mid-side nodes.
Purpose:  Define initial nodal point velocities for a node. 
*INITIAL_VELOCITY_NODE 
Card 
1 
Variable 
NID 
Type 
I 
2 
VX 
F 
Default 
none 
0. 
3 
VY 
F 
0. 
4 
VZ 
F 
0. 
5 
6 
7 
8 
VXR 
VYR 
VZR 
ICID 
F 
0. 
F 
0. 
F 
0. 
I 
0 
  VARIABLE   
DESCRIPTION
NID 
Node ID 
VX 
VY 
VZ 
VXR 
VYR 
VZR 
ICID 
Initial translational velocity in 𝑥-direction 
Initial translational velocity in 𝑦-direction 
Initial translational velocity in 𝑧-direction 
Initial rotational velocity about the 𝑥-axis 
Initial rotational velocity about the 𝑦-axis 
Initial rotational velocity about the 𝑧-axis 
Local  coordinate  system  ID.    The  specified  velocities  are  in  the
local system if ICID is greater than zero.  Furthermore, if ICID is
greater  than  zero,  *INCLUDE_TRANSFORM  does  not  rotate  the
initial velocity values specificied by VX, VY, …, VZR. 
See Remarks on *INITIAL_VELOCITY card.
*INITIAL 
Purpose:  Define the initial translational and rotational velocities at the center of gravity 
(c.g.)  for  a  rigid  body  or  a  nodal  rigid  body.    This  input  overrides  all  other  velocity 
input for the rigid body and the nodes which define the rigid body. 
Card 
1 
Variable 
PID 
Type 
I 
2 
VX 
F 
Default 
none 
0. 
3 
VY 
F 
0. 
4 
VZ 
F 
0. 
5 
6 
7 
8 
VXR 
VYR 
VZR 
ICID 
F 
0. 
F 
0. 
F 
0. 
I 
0 
  VARIABLE   
DESCRIPTION
PID 
VX 
VY 
VZ 
VXR 
VYR 
VZR 
ICID 
Part ID of the rigid body or the nodal rigid body. 
Initial translational velocity at the c.g.  in global 𝑥-direction. 
Initial translational velocity at the c.g.  in global 𝑦-direction. 
Initial translational velocity at the c.g.  in global 𝑧-direction. 
Initial rotational velocity at the c.g.  about the global 𝑥-axis. 
Initial rotational velocity at the c.g.  about the global 𝑦-axis. 
Initial rotational velocity at the c.g.  about the global 𝑧-axis. 
Local  coordinate  system  ID.    The  specified  velocities  are  in  the
local system if ICID is greater than zero.  Furthermore, if ICID is
greater  than  zero,  *INCLUDE_TRANSFORM  does  not  transform 
the initial velocity values specificied by VX, VY, …, VZR. 
See remarks 3 and 4 on the *INITIAL_VELOCITY input description.
*INITIAL_VELOCITY_GENERATION 
Purpose:  Define initial velocities for rotating and translating bodies. 
NOTE:  Rigid  body  velocities  cannot  be  reinitialized  after 
dynamic  relaxation  by  setting  PHASE=1  since  rigid 
body velocities are always restored to the values that 
existed prior to dynamic relaxation.  Reinitialization 
of  velocities  after  dynamic  relaxation  is  only  availa-
ble for nodal points of deformable bodies; therefore, 
if rigid bodies are present  in the part set ID, this in-
put should be defined twice, once for PHASE=0 and 
again for PHASE=1. 
  Card 1 
Variable 
1 
ID 
2 
3 
STYP 
OMEGA 
Type 
I 
I 
F 
Default 
none 
none 
0. 
  Card 2 
Variable 
1 
XC 
Type 
F 
Default 
0. 
2 
YC 
F 
0. 
3 
ZC 
F 
0. 
4 
VX 
F 
0. 
4 
NX 
F 
0. 
5 
VY 
F 
0. 
5 
NY 
F 
0. 
  VARIABLE   
DESCRIPTION
6 
VZ 
F 
0. 
6 
NZ 
F 
0. 
7 
8 
IVATN 
ICID 
I 
0 
7 
I 
0 
8 
PHASE 
IRIGID 
I 
0 
I 
0 
ID 
Part ID, part set ID, or node set ID.  If zero, STYP is ignored, and
all  velocities  are  set.    WARNING  if  IVATN = 0:  If  a  part  ID  of  a 
rigid body is specified only the nodes that belong to elements of
the rigid body are initialized.  Nodes defined under the keyword.
  Set 
initialized. 
*CONSTRAINED_EXTRA_NODES  are  not 
IVATN = 1 to initialize velocities of slaved nodes and parts.
VARIABLE   
DESCRIPTION
STYP 
Set type.  See Remark 5. 
EQ.1: part set ID, see *SET_PART, 
EQ.2: part ID, see *PART, 
EQ.3: node set ID, see *SET_NODE. 
OMEGA 
Angular velocity about the rotational axis. 
VX 
VY 
VZ 
Initial translational velocity in 𝑥-direction . 
Initial translational velocity in 𝑦-direction .   
Initial translational velocity in 𝑧-direction .   
IVATN 
Flag for setting the initial velocities of slave nodes and parts: 
EQ.0: slaved parts are ignored. 
EQ.1: slaved parts and slaved nodes of the master parts will be
assigned initial velocities like the master part. 
Local coordinate system ID.  The specified translational velocities
(VX,  VY,  VZ)  and  the  direction  cosines  of  the  rotation  axis  (NX,
NY, NZ) are in the global system if ICID = 0 and are in the local 
system  if  ICID  is  defined.    Therefore,  if  ICID  is  defined, 
*INCLUDE_TRANSFORM  does  not transform  (VX,  VY,  VZ)  and
(NX, NY, NZ).  
Global 𝑥-coordinate on rotational axis. 
Global 𝑦-coordinate on rotational axis. 
Global 𝑧-coordinate on rotational axis. 
𝑥-direction  cosine.    If  set  to  -999,  NY  and  NZ  are  interpreted  as 
the 1st and 2nd nodes defining the rotational axis, in which case the
coordinates  of  node  NY  are  used  as  XC,  YC,  ZC.    If  ICID  is
defined,  the  direction  cosine,  (NX,  NY,  NZ),  is  projected  along
coordinate  system  ICID  to  yield  the  direction  cosines  of  the 
rotation axis only if NX ≠ -999. 
𝑦-direction  cosine  or  the  1st  node  of  the  rotational  axis  when 
NX = -999. 
ICID 
XC 
YC 
ZC 
NX 
NY
NZ 
*INITIAL_VELOCITY_GENERATION 
DESCRIPTION
𝑧-direction  cosine  or  the  2nd  node  of  the  rotational  axis  when 
NX = -999. 
PHASE 
Flag specifying phase of the analysis the velocities apply to: 
EQ.0: Velocities are applied immediately, 
EQ.1: Velocities  are  applied  after  reaching  the  start  time,
STIME,  which  is  after  dynamic  relaxation,  if  active,  is
completed.    See  the  keyword:  *INITIAL_VELOCITY_-
GENERATION_START_TIME.  STIME defaults to zero. 
Controls hierarchy of initial velocities set with *INITIAL_VELOC-
ITY_GENERATION  versus  those  set  with  *PART_INERTIA / 
*CONSTRAINED_NODAL_RIGID_BODY_INERTIA  when 
the 
commands conflict. 
EQ.0: *PART_INERTIA /  *CONSTRAINED_NODAL_RIGID_-
BODY_INERTIA controls initial velocities.  
EQ.1: *INITIAL_VELOCITY_GENERATION  controls 
velocities.  This option does not apply if STYP = 3. 
initial 
IRIGID 
Remarks: 
1.  Exclusions.  This generation input must not be used with *INITIAL_VELOCI-
TY or *INITIAL_VELOCITY_NODE options. 
2.  Order Dependence.  The velocities are initialized in the order the *INITIAL_-
VELOCITY_GENERATION input is defined.  Later input via the *INITIAL_VE-
LOCITY_GENERATION keyword may overwrite the velocities previously set. 
3.  Consistency for Rigid Body Nodes.  Nodes which belong to rigid bodies must 
have motion consistent with the translational and rotational velocity of the rigid 
body.    During  initialization  the  rigid  body  translational  and  rotational  rigid 
body  momentum's  are  computed  based  on  the  prescribed  nodal  velocities.  
From  this  rigid  body  motion  the  velocities  of  the  nodal  points  are  computed 
and reset to the new values.  These new values may or may not be the same as 
the values prescribed for the node. 
4.  SPH.  SPH elements can be initialized using the STYP=3 option only.  
5.  Constrained  Nodal  Rigid  Bodies.    Part  IDs  of  *CONSTRAINED_NODAL_-
RIGID_BODYs  that  do  not  include  the  INERTIA  option  are  not  recognized  by
the code in the case of STYP=1 or 2.  Use STYP=3 (a node set ID) when initializ-
ing velocity of such nodal rigid bodies.
*INITIAL_VELOCITY_GENERATION_START_TIME 
Purpose:    Define  a  time  to  initialize  velocities  after  time  zero.    Time  zero  starts  after 
dynamic relaxation if used for initialization.    
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
STIME 
Type 
F 
Default 
0.0 
  VARIABLE   
DESCRIPTION
STIME 
Start time. 
Remarks: 
1.  Only  one 
*INITIAL_VELOCITY_GENERATION_START_TIME 
can  be 
specified.  Multiple start times are not allowed. 
2.  All  *INITIAL_VELOCITY_GENERATION  commands  adhere  to  the  start  time 
provided  the  requirement  is  met  that  at  least  one  of  those  commands  has 
PHASE set to 1. 
3.  When  *INITIAL_VELOCITY_GENERATION_START_TIME  is  active,  nodes 
that  are  not  part  of  the  initial  velocity  generation  definitions  will  be  re-
initialized with velocities as they were at 𝑡 = 0.
Available options include: 
PART 
SET 
*INITIAL 
Purpose:    Define  initial  voided  part  set  ID’s  or  part  numbers.    This  command  can  be 
used only when ELFORM = 12 in *SECTION_SOLID.  Void materials cannot be created 
during the calculation.  Fluid elements which are evacuated, e.g., by a projectile moving 
through the fluid, during the calculation are approximated as fluid elements with very 
low  densities.    The  constitutive  properties  of  fluid  materials  used  as  voids  must  be 
identical  to  those  of  the  materials  which  will  fill  the  voided  elements  during  the 
calculation.    Mixing  of  two  fluids  with  different  properties  is  not  permitted  with  this 
option.   
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PSID/PID 
Type 
I 
Default 
none 
Remark 
1 
  VARIABLE   
DESCRIPTION
PSID/PID 
Part set ID or part ID, see also *SET_PART: 
Remarks: 
This  void  option  and  multiple  materials  per  element,  see  *ALE_MULTI-MATERIAL_-
GROUP are incompatible and cannot be used together in the same run.
*INITIAL_VOLUME_FRACTION_OPTION 
Available option: 
NALEGP 
Purpose:    Define  initial  volume  fractions  of  different  materials  in  multi-material  ALE 
elements.    Without  NALEGP  option,  the  keyword  allows  up  to  7  ALE  multi-material 
groups.  The NALEGP option adds in an additional card immediately after the keyword 
to  let  users  input  the  number  of  ALE  multi-material  groups  to  be  read  in  for  each 
element. 
Format without NALEGP option: 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EID 
VF1 
VF2 
VF3 
VF4 
VF5 
VF6 
VF7 
Type 
I 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Card  1  repeated  multiple  times.    Each  card  for  an  ALE  element  volume  fraction 
information. 
Format with NALEGP option: 
NALEGP Card.  Additional card for the NALEGP keyword option. 
 Optional 
1 
Variable 
NALEGP 
Type
Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EID 
VF1 
VF2 
VF3 
VF4 
VF5 
VF6 
VF7 
Type 
I 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 1a 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VF8 
VF9 
VF10 
VF11 
VF12 
VF13 
VF14 
VF15 
Type 
I 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
… 
  Card 1z 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  VF(NGP-2)  VF(NGP-1)  VF(NGP) 
Type 
I 
F 
F 
Default 
none 
0.0 
0.0 
Card 1 is continued by additional cards until all the NALEGP volume fractions for this 
element  are  listed.    Card  1  and  its  continuation  cards  are  repeated  until  all  ALE 
elements are finished. 
  VARIABLE   
DESCRIPTION
EID 
VF1 
VF2 
Element ID. 
Volume fraction of multi-material group 1, AMMGID = 1. 
Volume  fraction  of  multi-material  group  2.    Only  needed  in 
simulations with 3 material groups.  Otherwise VF2 = 1 − VF1.
*INITIAL_VOLUME_FRACTION 
DESCRIPTION
VF3 
VF4 
VF5 
VF6 
VF7 
Volume fraction of multi-material group 3, AMMGID = 3. 
Volume fraction of multi-material group 4, AMMGID = 4. 
Volume fraction of multi-material group 5, AMMGID = 5.    
Volume fraction of multi-material group 6, AMMGID = 6. 
Volume fraction of multi-material group 7, AMMGID = 7. 
VF(N) 
Volume fraction of multi-material group N, AMMGID = N.
*INITIAL_VOLUME_FRACTION_GEOMETRY 
Purpose:  This is a volume-filling command for defining the volume fractions of various 
ALE multi-material groups (AMMG) that initially occupy various spatial regions in an 
ALE  mesh.    This  applies  only  to  ELFORMs  11  and  12  in  *SECTION_SOLID  and  ALE-
FORM 11 in  *SECTION_ALE2D.  For ELFORM 12, AMMGID 2 is void.  See Remark 2. 
Background ALE Mesh Card.  Defines the background ALE mesh set & an AMMGID 
that initially fills it.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FMSID 
FMIDTYP  BAMMG  NTRACE 
Type 
I 
Default 
none 
I 
0 
I 
0 
I 
3 
  VARIABLE   
FMSID 
DESCRIPTION
A  background  ALE  (fluid)  mesh  SID  to  be  initialized  or  filled
with  various  AMMG’s.    This  set  ID  refers  to  one  or  more  ALE
parts. 
FMIDTYP 
ALE mesh set ID type: 
EQ.0: FMSID is an ALE part set ID (PSID). 
EQ.1: FMSID is an ALE part ID (PID). 
BAMMG 
NTRACE 
The background fluid group ID or ALE Multi-Material group ID 
(AMMGID)  that  initially  fills  all  ALE  mesh  region  defined  by
FMSID. 
Number  of  sampling  points  for  volume  filling  detection.
Typically  NTRACE  ranges  from  3  to  maybe  10  (or  more).    The
higher  it  is,  the  finer  the  ALE  element  is  divided  so  that  small
gaps between 2 Lagrangian shells may be filled in.  See Remark 4.
Pairs of Container Cards. 
For each container include one “Container Card” (Card a) and one geometry card (Card 
bi).  Include as many pairs as desired.  This input ends at the next keyword (“*”) card.
Contained  Card.    Defines  the  container  type  and  the  AMMGID  that  fills  the  region 
defined by the container type.  
  Card a 
1 
2 
3 
Variable 
CNTTYP 
FILLOPT 
FAMMG 
Type 
I 
Default 
none 
I 
0 
I 
none 
7 
8 
4 
VX 
F 
0 
5 
VY 
F 
0 
6 
VZ 
F 
0 
DESCRIPTION
  VARIABLE   
CNTTYP 
A “container” defines a Lagrangian surface boundary of a spatial
region,  inside  (or  outside)  of  which,  an  AMMG  would  fill  up.
CNTTYP  defines  the  container  geometry  type  of  this  surface
boundary (or shell structure). 
EQ.1: The container geometry is defined by a part ID (PID) or a 
part set ID (PSID), where the parts should be defined by
shell elements . 
EQ.2: The  container  geometry  is  defined  by  a  segment  set
(SGSID). 
EQ.3: The  container  geometry  is  defined  by  a  plane:  a  point
and a normal vector. 
EQ.4: The container geometry is defined by a conical surface: 2
end points and 2 corresponding radii (in 2D see Remark 
6). 
EQ.5: The  container  geometry  is  defined  by  a  cuboid  or
rectangular  box:  2  opposing  end  points,  minimum  to 
maximum coordinates. 
EQ.6: The  container  geometry  is  defined  by  a  sphere:  1  center
point, and a radius.
VARIABLE   
FILLOPT 
FAMMG 
DESCRIPTION
A flag to indicate which side of the container surface the AMMG
is  supposed  to  fill.    The  “head”  side  of  a  container  sur-
face/segment is defined as the side pointed to by the heads of the
normal  vectors  of  the  segments  (“tail”  side  refers  to  opposite
direction to “head”).  See Remark 5. 
EQ.0: The  “head”  side  of  the  geometry  defined  above  will  be
filled with fluid (default). 
EQ.1: The  “tail”  side  of  the  geometry  defined  above  will  be
filled with fluid. 
This  defines  the  fluid  group  ID or  ALE  Multi-Material  group  ID 
(AMMGID) which will fill up the interior (or exterior) of the space
defined by the “container”. The order of AMMGIDs is determined by 
the  order  in  which  they  are  listed  under  *ALE_MULTI-MATERIAL_-
GROUP  card.    For  example,  the  first  data  card  under  the  *ALE_-
MULTI-MATERIAL_GROUP keyword defines the multi-material 
group with ID (AMMGUD) 1, the second data card defined AM-
MGID = 2 and so on. 
LT.0:  | 
| 
FAMMG 
*SET_MULTI-
MATERIAL_GROUP_LIST  id  listing  pairs  of  group  IDs.
For each    pair,  the  2nd group replaces  the  first  one  in  the 
“container”. 
is 
a 
VX 
VY 
VZ 
Initial velocity in the global 𝑥-direction for this AMMGID. 
Initial velocity in the global 𝑦-direction for this AMMGID. 
Initial velocity in the global 𝑧-direction for this AMMGID.
Part/Part Set Container Card.  Additional card for CNTTYP = 1. 
  Card b1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
STYPE  NORMDIR
XOFFST 
Type 
I 
Default 
none 
I 
0 
I 
0 
F 
0.0 
Remark 
obsolete
  VARIABLE   
SID 
DESCRIPTION
A  Set  ID  pointing  to  a  part  ID  (PID)  or  part  set  ID  (PSID)  of  the
Lagrangian  shell  element  structure  defining  the  “container”
geometry to be filled . 
SSTYPE 
Set ID type: 
EQ.0: Container SID is a Lagrangian part set ID (PSID). 
EQ.1: Container SID is a Lagrangian part ID (PID). 
NORMDIR 
Obsolete . 
XOFFST 
Absolute  length  unit  for  offsetting  the  fluid  interface  from  the
nominal  fluid  interface  LS-DYNA  would  otherwise  define  by 
default.    This  parameter  only  applies  to  GEOTYPE = 1  (4th
column)  and  GEOTYPE = 2  (3rd  column).    This  is  applicable  to 
cases in which high pressure fluid is contained within a container.
The offset allows LS-DYNA time to prevent leakage.  In general, 
this may be set to roughly 5-10% of the ALE elm width.  It may be 
important  only  for  when  ILEAK  is  turned  ON  to  give  the  code
time to "catch" the leakage.  If ILEAK is not ON, this may not be
necessary.
Segment Set Container Card.  Additional card for CNTTYP = 2. 
  Card b2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SGSID  NORMDIR  XOFFST 
Type 
I 
Default 
none 
I 
0 
F 
0.0 
Remark 
obsolete 
  VARIABLE   
DESCRIPTION
SGSID 
Segment Set ID defining the “container”, see *SET_SEGMENT. 
NORMDIR 
Obsolete . 
XOFFST 
Absolute  length  unit  for  offsetting  the  fluid  interface  from  the
nominal  fluid  interface  LSDYNA  would  otherwise  define  by
default.    This  parameter  only  applies  to  GEOTYPE = 1  (4th
column)  and  GEOTYPE = 2  (3rd  column).    This  is  applicable  to 
cases in which high pressure fluid is contained within a container.
The offset allows LS-DYNA time to prevent leakage.  In general, 
this may be set to roughly 5-10% of the ALE elm width.  It may be 
important  only  for  when  ILEAK  is  turned  ON  to  give  the  code
time to "catch" the leakage.  If ILEAK is not ON, this may not be
necessary. 
Plane Card.  Additional card for CNTTYP = 3. 
  Card b3 
Variable 
1 
X0 
Type 
F 
2 
Y0 
F 
3 
Z0 
F 
4 
5 
6 
7 
8 
XCOS 
YCOS 
ZCOS 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none
VARIABLE   
DESCRIPTION
X0, Y0, Z0 
𝑥, 𝑦 and 𝑧 coordinate of a spatial point on the plane. 
XCOS, YCOS, ZCOS 
𝑥, 𝑦 and 𝑧 direction cosines of the plane normal vector.  The
filling  will  occur  on  the  side  pointed  to  by  the  plane
normal vector (or “head” side). 
Cylinder/Cone Container Card.   Additional Card for CNTTYP = 4 . 
  Card b4 
Variable 
1 
X0 
Type 
F 
2 
Y0 
F 
3 
Z0 
F 
4 
X1 
F 
5 
Y1 
F 
6 
Z1 
F 
7 
R1 
F 
8 
R2 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
X0, Y0, Z0 
𝑥, 𝑦 and 𝑧 coordinate of the center of the 1st base of the cone. 
X1, Y1, Z1 
𝑥, 𝑦 and 𝑧 coordinate of the center of the 2nd base of the cone. 
R1 
R2 
Radius of the 1st base of the cone 
Radius of the 2nd base of the cone 
Rectangular Box Container Card.  Additional Card for CNTTYP = 5. 
  Card b5 
Variable 
1 
X0 
Type 
F 
2 
Y0 
F 
3 
Z0 
F 
4 
X1 
F 
5 
Y1 
F 
6 
Z1 
F 
7 
8 
LCSID 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
X0, Y0, Z0 
Minimum 𝑥, 𝑦 and 𝑧 coordinates of the box.
VARIABLE   
DESCRIPTION
X1, Y1, Z1 
Maximum 𝑥, y and 𝑧 coordinates of the box. 
LCSID 
Local coordinate system ID, if defined, the box is aligned with the
local  coordinate  system  instead  of  global  coordinate  system.
Please see *DEFINE_COORDINATE_ for details. 
Sphere Container Card.  Additional card for CNTTYP = 6. 
5 
6 
7 
8 
  Card b6 
Variable 
1 
X0 
Type 
F 
2 
Y0 
F 
3 
Z0 
F 
4 
R0 
F 
Default 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
X0, Y0, Z0 
𝑥, 𝑦 and 𝑧 coordinate of the center of the sphere. 
R0 
Radius of the sphere 
Remarks: 
1.  Structure of Data Cards.  After card 1 defining the basic mesh filled by certain 
fluid  group  (AMMGID),  each  “filling  action”  will  require  2  additional  lines  of 
input (cards a, and b#, where # is the CNTTYP value).  At the minimum there 
will be 3 cards required for this command (1, a, and b#) for 1 “filling action”. 
There  can  be  one  or  more  “filling  actions”  prescribed  for  each  instance  of  this 
command.    The  “filling  actions”  take  place  in  the  prescribed  order  and  the  ef-
fects  are  cumulative.    Later  filling  actions  will  over-write  the  previous  ones.  
Therefore  any  complex  filling  logic  will  require  some  planning.    For  example, 
the following card sequence, with 2 “filing actions”, is allowable: 
*INITIAL_VOLIME_FRACTION_GEOMTRY 
[Card 1] 
[Card a, CNTTYP = 1] 
[Card b1]
[Card a, CNTTYP = 3] 
[Card b3] 
This  sequence  of  cards  prescribes  a  system  of  background  ALE  mesh  with  2 
“filing actions” to be executed.  The 1st is a filling of a CNTTYP = 1, and the 2nd 
of CNTTYP = 3. 
“Card  a”  is  required  for  all  container  geometry  types  (CNTTYP).    “Card  bi” 
defines the container actual geometry and corresponds to each of the CNTTYP 
choice. 
2.  Group  IDs  for  ELFORM  12.    If  ELFORM=12,  the  single-material-and-void 
element forumation, is used in *SECTION_SOLID, then the non-void material is 
defaults  to  AMMG = 1  and  the  void  to  AMMG = 2.    These  multi-material 
groups are implied even though no *ALE_MULTI-MATERIAL_GROUP card is 
required. 
3.  Using Shells to Divide Space.  A simple ALE background mesh (for example, 
a cuboid mesh) can be constructed enveloping some Lagrangian shell structure 
(or  container).    The  ALE  region  inside  this  Lagrangian  shell  container  may  be 
filled  with  one  multi-material  group  (AMMG1),  and  the  outside  region  with 
another (AMMG2).  This approach simplifies the mesh generation requirements 
for ALE material parts with complex geometries. 
4.  NTRACE.  Default is NTRACE=3 in which case the total number is  
(2 × NTRACE + 1)3 = 73 
This means an ALE element is subdivided into 7 × 7 × 7 regions.  Each is to be 
filled in with the appropriate AMMG.  An example of this application would be 
the filling of initial gas between multiple layers of Lagrangian airbag shell ele-
ments sharing the same ALE element. 
5. 
Interior/Exterior Fill Setting.  To set which side of a container is to be filled: (1) 
define the shell (or segment) container with inward normal vectorsl; then (2) set 
the  FILLOPT  field on  “Card a” to 0, corresponding to the head of  the normal, 
for the interior, and to 1, corresponding to the tail of the normal, for the exteri-
or. 
6.  Two  Dimensional  Geometry.    If  the  ALE  model  is  2D  (*SECTION_ALE2D 
instead  of  *SECTION_SOLID),  CNTTYP=4  defines  a  quadrangle.    In  this  case 
the fields which, in the 3D case define a cone, are interpreted as the corner co-
ordinates of a clockwise defined (inward normal) quadrangle having the verti-
ces: (X1, Y1 ),  (X2, Y2), (X3, Y3), and (X4, Y4).  The CNTYPE = 4 input fields X0, 
Y0,  Z0, X1,  Y1, Z1,  R1,  and  R2  becomes  X1, Y1,  X2, Y2,  X3, Y3,  X4,  and  Y4  re-
spectively.  CNTTYP=6 should be used to fill a circle.
Example: 
Consider  a  simple  ALE  model  with  ALE  parts  H1-H5  (5  AMMGs  possible)  and  1 
Lagrangian shell (container) part S6.  Only parts H1 and S6 initially have their meshes 
defined.  We will perform 4 “filling actions”.  The volume filling results after each step 
will be shown below to clarify the concept used.  The input for the volume filling looks 
like this. 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
$ H1 = AMMG 1 = fluid 1 initially occupying whole ALE mesh= background mesh 
$ H5 = AMMG 5 = fluid 5 fills below a plane = filling action 1 = CNTTYP=3 
$ H2 = AMMG 2 = fluid 2 fills outside S5    = filling action 2 = CNTTYP=1 
$ H3 = AMMG 3 = fluid 3 fills inside a cone = filling action 3 = CNTTYP=4 
$ H4 = AMMG 4 = fluid 4 fills inside a box  = filling action 4 = CNTTYP=5 
$ S6 =          Lagrangian shell container 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
*ALE_MULTI-MATERIAL_GROUP 
         1         1 
         2         1 
         3         1 
         4         1 
         5         1 
*INITIAL_VOLUME_FRACTION_GEOMETRY 
$ The 1st card fills the whole pid H1 with AMMG 1=background ALE mesh 
$    FMSID   FMIDTYP     BAMMG     <=== card 1: background fluid 
         1         1         1 
$ filling action 1 = AMMG 5 fill all elms below a plane   
$ CNTTYPE   FILLOPT FILAMMGID     <=== card a  : container: CNTTYPE=3=plane 
         3         0         5 
$   X0, Y0,   Z0,    NX,  NY, NZ   <=== card b-3: details on container =plane 
  25.0,20.0, 0.0,   0.0,-1.0,0.0 
$ filling action 2: AMMG 2 fills OUTSIDE (FILLOPT=1) shell S6 (inward normals);  
$ CNTTYPE   FILLOPT     FAMMG  <== card a  : container #1; FILLOPT=1=fill tail 
         1         1         2 
$    SETID   SETTYPE   NORMDIR  <== card b-1: details on container #1 
         6         1         0 
$ filling action 3 = AMMG 3 fill all elms inside a CONICAL region 
$ CNTTYPE   FILLOPT     FAMMG  CNTTYP = 4 = Container = conical region 
         4         0         3 
$       X1        Y1        Z1        X2        Y2        Z2        R1       R2 
      25.0      75.0       0.0      25.0      75.0       1.0       8.0      8.0 
$ filling action 4 = AMMG 4 fill all elms inside a BOX region 
$ CNTTYPE   FILLOPT  FFLUIDID                 : CNTTYP=5 = "BOX"  
         5         0         4 
$     XMIN      YMIN      ZMIN      XMAX      YMAX      ZMAX 
      65.0      35.0       0.0      85.0      65.0       1.0 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8
Before  the  1st  “filling  action”  the  whole  ALE  mesh  of  part  H1  is  filled  with  AMMG  1 
(white).  After the 1st “filling action”, AMMG 5 fills below the specified plane. 
After the 1st and 2nd “filling actions”, it fills outside the shell (S6) with AMMG 2.
After the 1st, 2nd and 3rd “filling actions”, it fills in the analytical sphere with AMMG 3. 
After the 1st, 2nd, 3rd and 4th “filling actions”, it fills in the analytical box with AMMG 4.
In  this  section  the  user  defined  integration  rules  for  beam  and  shell  elements  are 
specified.    IRID  refers  to  integration  rule  identification  number  on  *SECTION_BEAM 
and *SECTION_SHELL cards respectively.  Quadrature rules in the *SECTION_SHELL 
and *SECTION_BEAM cards need to be specified as a negative number.  The absolute 
value of the negative number refers to user defined integration rule number.  Positive 
rule  numbers  refer  to  the  built  in  quadrature  rules  within  LS-DYNA.    The  keyword 
cards in this section are: 
*INTEGRATION_BEAM 
*INTEGRATION_SHELL
*INTEGRATION_BEAM 
Purpose:  To support user defined through the thickness integration rules for the beam 
element. 
  Card 1 
1 
Variable 
IRID 
Type 
I 
Default 
none 
2 
NIP 
I 
0 
3 
RA 
F 
0.0 
4 
ICST 
I 
0 
5 
K 
I 
0 
6 
7 
8 
Standard Cross-Section Card.  Additional card for ICST > 0.  
Card 
Variable 
1 
D1 
Type 
F 
2 
D2 
F 
3 
D3 
F 
4 
D4 
F 
5 
6 
SREF 
TREF 
F 
F 
7 
D5 
F 
8 
D6 
F 
Default 
none 
none 
none 
none 
0.0 
0.0 
none 
none 
Quadrature Cards.  Include NIP additional cards below for NIP ≠ 0.  
Card 
Variable 
Type 
1 
S 
F 
2 
T 
F 
3 
WF 
4 
PID 
F 
I 
5 
6 
7 
8 
  VARIABLE   
IRID 
DESCRIPTION
Integration  rule  ID.    IRID  refers  to  IRID  on  *SECTION_BEAM 
card. 
NIP 
Number of integration points, see also ICST.
st
tt
Thicknesses defined on beam
cross-section cards
Relative Area = 
st × tt
Figure 24-1.  Definition of relative area for user defined integration rule. 
  VARIABLE   
RA 
DESCRIPTION
Relative  area  of  cross  section,  i.e.,  the  actual  cross-sectional  area 
divided  by  the  area  defined  by  the  product  of  the  specified
thickness  in  the  s  direction  and  the  thickness  in  the  t  direction. 
See also ICST below and Figure 24-1. 
ICST 
Standard  cross  section  type,  ICST.    If  this  type  is  nonzero  then
NIP  and  the  relative  area  above  should  be  input  as  zero.    See 
shapes in Figure 24-2 following Remarks. 
EQ.01:  I-Shape 
EQ.02:  Channel 
EQ.03:  L-shape 
EQ.04:  T-shape 
EQ.05:  Tubular box 
EQ.06:  Z-Shape 
EQ.07:  Trapezoidal 
EQ.08:  Circular 
EQ.09:  Tubular 
EQ.10:  I-Shape 2 
EQ.11:  Solid Box 
EQ.12:  Cross 
EQ.13:  H-Shape 
EQ.14:  T-Shape 2 
EQ.15:  I-Shape 3 
EQ.16:  Channel 2 
EQ.17:  Channel 3 
EQ.18:  T-Shape 3 
EQ.19:  Box-Shape 2 
EQ.20:  Hexagon 
EQ.21:  Hat-Shape 
EQ.22:  Hat-Shape 2
A1
A2
A3
A12
A11
A10
A5
A4
A6
A7
A8
A9
 Figure 24-2.  Definition of integration points for user defined integration rule.
  VARIABLE   
DESCRIPTION
K 
Integration refinement parameter for standard cross section types.
Select an integer ≥ 0.  See Figure below. 
D1-D6 
Cross-section dimensions.  See Figure below. 
SREF 
TREF 
S 
T 
WF 
sref, location of reference surface normal to s, for the Hughes-Liu 
beam only.  This option is only useful if the beam is connected to
a shell or another beam on its outer surface.  Overrides NSLOC in
*SECTION_BEAM even if SREF = 0. 
tref, location of reference surface normal to t, for the Hughes-Liu 
beam only.  This option is only useful if the beam is connected to
a shell or another beam on its outer surface.  Overrides NTLOC in 
*SECTION_BEAM even if TREF = 0. 
Normalized s coordinate of integration point, −1 ≤ 𝑠 ≤ 1. 
Normalized t coordinate of integration point, −1 ≤ 𝑡 ≤ 1. 
Weighting  factor,  Ari 
integration  point  divided  by  actual  cross  sectional  area
the  area  associated  with  the 
,  i.e.,
𝐴𝑟𝑖 =
𝐴𝑖
⁄ , see Figure 24-1.
DESCRIPTION
Optional  PID,  used  to  identify  material  properties  for  this
integration  point.    If  zero,  the  “master”  PID  (referenced  on
*ELEMENT)  will  be  used.    This  feature  will  be  available  in
release 3 of version 971. 
  VARIABLE   
PID 
Remarks: 
The  input  for  standard  beam  section  types  is  defined  below.    In  following  figures  the 
dimensions are shown on the left and the location of the integration points are shown 
on the right.  If a quantity is not defined in the sketch, then it should be set to zero in the 
input.  The input quantities include: 
  D1 - D6   =   Dimensions of section 
k   =   Integration refinement parameter ( an integer GE.  0) 
sref   =   location of reference surface normal to s, Hughes-Liu beam only 
tref   =   location of reference surface normal to t, Hughes-Liu beam only 
D3
D1
(a)
D2
D4
2k+4
2k+3
4k+7
6k+9
4k+6
15
16
17
18
19
20
21
10 11
12 13 14
(b)
(c)
Figure  24-3.    Type  1:  I-Shape.    (a)  Cross  section  geometry.    (b)  Integration
point numbering.  (c) Example for k = 2.
D4
D3
D1
(a)
D2
2k+7
3k+9
k+4
k+3
2k+6
11
12
13
14
15
10
(b)
(b)
Figure  24-4.    Type  2:  Channel.    (a)  Cross  section  geometry.    (b)  Integration
point numbering.  (c) Example for k = 2.
D4
D3
K+2
D2
K+3
K+4
2K+5
D1
(a)
(b)
(c)
Figure  24-5.    Type  3:  L-shape.    (a)  Cross  section  geometry.    (b)  Integration
point numbering.  (c) Example for k = 2. 
D3
D1
(a)
D4
D2
k+2 k+3 k+4
2k+6
2k+5
3 4
4k+9
(b)
6 7 8 9
10
11
12
13
14
15
16
17
(c)
Figure  24-6.    Type  4:  T-shape.    (a)  Cross  section  geometry.    (b)  Integration
point numbering.  (c) Example for k = 2.
D3
D2
D1
(a)
2k+7
k+3
3k+8
D4
3k+7
k+4
4k+8
2k+6
11
12
13
14
15
16
10
(b)
(c)
Figure  24-7.   Type  5: Box-shape.   (a)  Cross section  geometry.  (b)  Integration
point numbering.  (c) Example for k = 2. 
D4
D3
D2
D1
(a)
k+3
2k+7
k+4
3k+9
2k+6
(b)
1 2 3 4 5
11
12
13
14
15
10
(c)
6789
Figure  24-8.    Type  6:  Z-shape.    (a)  Cross  section  geometry.    (b)  Integration
point numbering.  (c) Example for k = 2.
D3
D4
D1
(a)
(0,0)
(i,j)
(0,k+3)
[i×(k+3)+j]+1
(0,k+3)
(k+3,k+3)
1 2 3 4 5
9 10
11 12 13 14 15
18
20
23
25
19
24
17
22
16
21
(b)
(c)
Figure 24-9.  Type 7: Trapezoidal.  (a) Cross section geometry.  (b) Integration
point numbering.  (c) Example for k = 2. 
D1
j = k+3
(i,j)
j = 0
i = 0
i = 4(k+3)
[j×4(k+3)+i]+1
82
62
22
42
20
21
40
81
61
41
60 80 100
(a)
(b)
(c)
Figure  24-10.    Type  8:  Circular.    (a)  Cross  section  geometry.    (b)  Integration
point numbering.  (c) Example for k = 2.
D1
D2
j = k+3
(i,j)
j = 0
i = 0
i = 4(k+3)
[j×4(k+3)+i]+1
20
82
62
42
22
21
40
41
61
81
60 80 100
(a)
(b)
(c)
Figure  24-11.    Type  9:  Tubular.    (a)  Cross  section  geometry.    (b)  Integration
point numbering.  (c) Example for k = 2. 
D6
D5
D3
D2
(a)
2k+3
D4
D1
4k+7
6k+9
2k+4
4k+6
15
16
17
18
19
20
21
8 9 10 1112 13 14
(b)
(c)
Figure 24-12.  Type 10: I-Shape 2.  (a) Cross section geometry.  (b) Integration
point numbering.  (c) Example for k = 2.
D2
D1
(a)
(0,k+3)
(k+3,k+3)
[i×(k+3)+j]+1
(i,j)
(0,0)
(0,k+3)
(b)
21
16
11
22
17
12
24
19
14
25
20
15
10
23
18
13
(c)
Figure 24-13.  Type 11: Solid Box.  (a) Cross section geometry.  (b) Integration
point numbering.  (c) Example for k = 2. 
D4
2k+5
4k+9
5k+9
5k+10 6k+10
7k+11
6k+11
8k+12 7k+12
17 18 19
20 21 22
D3
D1/2
D1/2
D2
(a)
2k+4 4k+8
(b)
25 24 23
28
26
27
10
11
12
13
14
15
16
(c)
Figure  24-14.    Type  12:  Cross.    (a)  Cross  section  geometry.    (b)  Integration
point numbering.  (c) Example for k = 2.
D2/2
D4
D2/2
2k+6
D3
4k+11
6k+13
2k+5
4k+10
19 20 2122 23 24 25
10
11
12
13
14
15
16
17
18
D1
(a)
(b)
(c)
Figure 24-15.  Type 13: H-Shape.  (a) Cross section geometry.  (b) Integration
point numbering.  (c) Example for k = 2. 
D3
+
4k+9
6k+12
1718 19 20 212223 24
D1
6k+13
8k+16
2526 2728 2930 3132
+
+
(b)
(c)
10
11
12
13
14
15
16
D4
(a)
D2
Figure 24-16.  Type 14: T-Shape 2.  (a) Cross section geometry.  (b) Integration 
point numbering.  (c) Example for k = 2.
D1/2
D4
D2
(a)
2k+4
1 2 3 4 5 6 7 8
D1/2
D3
4k+9 6k+12
6k+11 8k+4
17
18
19
20
21
22
23
24
25
26
27
28
29
30
2k+5
4k+8
9 10 11 12 13 14 15 16
(b)
(c)
Figure 24-17.  Type 15: I-Shape 3.  (a) Cross section geometry.  (b) Integration 
point numbering.  (c) Example for k = 2. 
D3
D2
D1
D3
2k+7
3k+10
k+3
3k+9 4k+12
k+4
2k+6
11
12
13
14
15
16
17
18
19
20
10
(a)
(b)
(c)
Figure 24-18.  Type 16: Channel 2.  (a) Cross section geometry.  (b) Integration
point numbering.  (c) Example for k = 2.
D1
D3
D1
D4
(a)
2k+4
4k+6
4k+5
D2
6k+7
2k+3
10
11
12
13
14
15
16
17
18
19
(b)
(c)
Figure 24-19.  Type 17: Channel 3.  (a) Cross section geometry.  (b) Integration
point numbering.  (c) Example for k = 2. 
D2
D4
D1
(a)
4k+9 6k+11
6k+10 8k+12
17
18
19
20
21
22
23
24
25
26
27
28
D3
2k+5
2k+4
4k+8
1 2 3 4 5 6 7 8
9 10 11 12 13 14 15 16
(b)
(c)
Figure 24-20.  Type 18: T-Shape 3.  (a) Cross section geometry.  (b) Integration
point numbering.  (c) Example for k = 2.
D6
D2
D3
D4
D1
(a)
D5
2k+7
k+3
3k+8
3k+7
k+4
4k+8
2k+6
11
12
13
14
15
16
10
(b)
(c)
Figure  24-21.    Type  19:  Box  Shape  2.    (a)  Cross  section  geometry.    (b)
Integration point numbering.  (c) Example for k = 2. 
D1
(0,0)
(0,k+3)
(i,j)
(0,k+3)
[i×(k+3)+j]+1
(k+3,k+3)
(k+3) 2+
          [i×(k+3)+j]+1
The bottom half
is the reflection of
the top-half with
ids offset by (k+3)2
(b)
D3
D2
(a)
1 2 3 4 5
9 10
11 12 13 14 15
18
20
23
25
19
24
17
22
16
21
46
47
49
50
48
41 42 43 44 45
36 37 38 39 40
31 32 33 34 35
26 27 28 29 30
(c)
Figure 24-22.  Type 20: Hexagon.  (a) Cross section geometry.  (b) Integration
point numbering.  (c) Example for k = 2.
D1
D4
D2
D3
(a)
D4
4k+9
2k+4
6k+12
+
+
6k+11
+
8k+14
+
(b)
17
18
19
20
21
22
23
9 10 1112
(c)
24
25
26
27
28
29
30
16
15
14
13
Figure 24-23.  Type 21: Hat-Shape.  (a) Cross section geometry.  (b) Integration
point numbering.  (c) Example for k = 2. 
D2
D6
D4
D3
D1
(a)
4k+10
2k+5
6k+13
D6
+
+
6k+12
D5
8k+16
+
8k+15
+
14k+22
(b)
18
19
20
21
22
23
24
10 1112 13
25
26
27
28
29
30
31
17
16
15
14
32 33 34 35 36 37 38 39 40 41 42 43 44 45 46 47 48 49 50
(c)
Figure  24-24.    Type  22:  Hat-Shape  2.    (a)  Cross  section  geometry.    (b)
Integration point numbering.  (c) Example for k = 2.
*INTEGRATION 
Purpose:    Define  user  defined  through  the  thickness  integration  rules  for  the  shell 
element.    This  option  applies  to  three  dimensional  shell  elements  with  three  or  four 
nodes  (ELEMENT_SHELL  types  1-11  and  16)  and  to  the  eight  node  thick  shell  (ELE-
MENT_TSHELL).  See *PART_COMPOSITE for a simpler alternative to *PART + *SEC-
TION_SHELL + *INTEGRATION_SHELL. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IRID 
NIP 
ESOP 
FAILOPT 
Type 
I 
I 
I 
I 
Define NIP cards below if ESOP = 0.  
Card 
Variable 
Type 
1 
S 
F 
2 
WF 
3 
PID 
F 
I 
4 
5 
6 
7 
8 
  VARIABLE   
DESCRIPTION
IRID 
NIP 
ESOP 
Integration  rule  ID  (IRID  refers  to  IRID  on  *SECTION_SHELL 
card). 
Number of integration points 
Equal spacing of integration points option: 
EQ.0: integration points are defined below, 
EQ.1: integration  points  are  equally  spaced  through  thickness 
such that the shell is subdivided into NIP layers of equal
thickness.
s = 1
Δti
midsurface
Figure  24-25.    In  the  user  defined  shell  integration  rule  the  ordering  of  the
integration points is arbitrary. 
s = -1
  VARIABLE   
FAILOPT 
DESCRIPTION
Treatment  of  failure  when  mixing  different  constitutive  types,
which  do  and  do  not  include  failure  models,  through  the  shell
thickness.    For  example,  consider  the  case  where  a  linear 
viscoelastic material model, which does not have a failure option,
is  mixed  with  a  composite  model,  which  does  have  a  failure
option.    Note:  If  the  failure  option  includes  failure  based  on  the
time  step  size  of  the  element,  element  deletion  will  occur 
regardless of the value of  FAILOPT. 
EQ.0: Element is deleted when the layers which include failure,
fail. 
EQ.1: Element  failure  cannot  occur  since  some  layers  do  not
have a failure option. 
S 
WF 
Coordinate of integration point in range -1 to 1. 
Weighting  factor.    This  is  typically  the  thickness  associated  with
the  integration  point  divided  by  actual  shell  thickness,  i.e.,  the
Δ𝑡𝑖
𝑡   as  seen  in 
weighting  factor  for  the  ith  integration  point = 
Figure 24-25.
VARIABLE   
PID 
DESCRIPTION
Optional  part  ID  if  different  from  the  PID  specified  on  the
element  card.    The  average  mass  density  for  the  shell  element  is
based  on  a  weighted  average  of  the  density  of  each  layer  that  is
used  through  the  thickness.    When  modifying  the  constitutive
constants  through  the  thickness,  it  is  often  necessary  to  defined
unique part IDs without elements that are referenced only by the
user  integration  rule.    These  additional  part  IDs  only  provide  a
density  and  constitutive  constants  with  local  material  axes  (if
used) and orientation angles taken from the PID referenced on the
element card.  In defining a PID for an integration point, it is okay
to  reference  a  solid  element  PID.    The  material  type  through  the
thickness can vary.
Interface  definitions  may  be  used  to  define  surfaces,  nodal  lines,  and  nodal  points  for 
which  the  displacement  and  velocity  time  histories  are  saved  at  some  user  specified 
frequency.    This  data  may  then  used  in  subsequent  analyses  as  an  interface  ID  in  the 
*INTERFACE_LINKING_DISCRETE_NODE  as  master  nodes,  in  *INTERFACE_LINK-
ING_SEGMENT  as  master  segments  and  in  *INTERFACE_LINKING_EDGE  as  the 
master edge for a series of nodes.  This  capability is especially useful for studying the 
detailed  response  of  a  small  member  in  a  large  structure.    For  the  first  analysis,  the 
member  of  interest  need  only  be  discretized  sufficiently  that  the  displacements  and 
velocities  on  its  boundaries  are  reasonably  accurate.    After  the  first  analysis  is 
completed,  the  member  can  be  finely  discretized  in  the  region  bounded  by  the 
interfaces.    Finally,  the  second  analysis  is  performed  to  obtain  highly  detailed 
information in the local region of interest.  When beginning the first analysis, specify a 
name for the interface segment file using the Z = parameter on the LS-DYNA execution 
line.  When starting the second analysis, the name of the interface segment file created 
in the first run should be specified using the L = parameter on the LS-DYNA command 
line.    Following  the  above  procedure,  multiple  levels  of  sub-modeling  are  easily 
accommodated.    The  interface  file  may  contain  a  multitude  of  interface  definitions  so 
that a single run of a full model can provide enough interface data for many component 
analyses.  The interface feature represents a powerful extension of LS-DYNA’s analysis 
capabilities.  The keyword cards for this purpose are: 
*INTERFACE_COMPENSATION_NEW 
*INTERFACE_COMPONENT_OPTION 
*INTERFACE_LINKING_DISCRETE_NODE_OPTION 
*INTERFACE_LINKING_EDGE 
*INTERFACE_LINKING_SEGMENT 
*INTERFACE_SPRINGBACK_OPTION1_OPTION2 
Interface  definitions  may  also  be  employed  to  define  soil-structure  interfaces  in 
earthquake  analysis  involving  non-linear  soil-structure  interaction where  the  structure 
may  be  non-linear  but  the  soil  outside  the  soil-structure  interface  is  assumed  to  be 
linear.    Free-field  earthquake  ground  motions  are  required  only  at  the  soil-structure 
interface for such analysis.  The keyword cards for this purpose are: 
*INTERFACE_SSI 
*INTERFACE_SSI_AUX
*INTERFACE_SSI_STATIC
*INTERFACE_BLANKSIZE_{OPTION} 
Available options include: 
DEVELOPMENT 
INITIAL_TRIM 
INITIAL_ADAPTIVE 
SCALE_FACTOR 
SYMMETRIC_PLANE 
Purpose:  This keyword causes LS-DYNA to run a blank-size development calculation 
instead of a finite element calculation.  The input for this feature consists of (1) the result 
of a completed metal forming simulation, (2) the corresponding initial blank, and (3) the 
desired result from the simulation in the form of a boundary curve or full mesh.  From 
these inputs the *INTERFACE_BLANKSIZE method adjusts the initial blank so that the 
resulting formed piece more closely matches the target.  The blank’s starting geometry 
may  be  systematically  improved  by  iterating.    A  GUI  for  using  this  available  in  LS-
SPACE
Target curves (FILENAME1, target.xyz)
Reference surface 
(FILENAME13, ref4.k)
Final blank (FILENAME2, final.k)
Initial blank (FILENAME3, initial.k)
Modified initial blank boundary (trimcurves.ibo)
Reference surface 
(FILENAME4, ref3.k)
Figure  25-1.    Trim  curve  development  using  a  reference  surface.    See
Example II.
PrePost  as  of  version  4.2  under  APPLICATION  →  Metal  Forming  →  Blank  Size/Trim 
line. 
NOTE: When this card is present LS-DYNA does not proceed 
to the finite element simulation. 
This  keyword  requires  one  or  all  three  keyword  options,  each  corresponding  to  a 
different kind of forming operation: 
1.  DEVELOPMENT.    This  option  takes  as  its  target  either  a  full  mesh  or  a 
minimum  boundary.    It  adjusts  the  blank  so  that  he  product  more  closely  ap-
proximates the target.  The computed blank-boundary is written to a file called 
trimcurves.ibo, which contains a *DEFINE_CURVE_TRIM_3D keyword. 
2. 
3. 
INITIAL_TRIM.    This  option  adjusts  the  blank  so  that  trimming  and  mesh-
refinement are mapped back onto the initial blank. 
INITIAL_ADAPTIVE.    This  option  reads  in  (1)  the  input  mesh  for  a  flanging 
simulation  as  well  as  (2)  the  adapted  mesh  calculated  during  flanging  simula-
tion.  It maps the refinement back to the initial blank. 
Card set for *INITIAL_BLANKSIZE_DEVELOPMENT. 
Development Parameter Card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IOPTION 
IADAPT  MAXSIZE  REFERENC
SPACE  MAXGAP  ORIENT 
Type 
I 
Default 
-2 
I 
1 
F 
I 
F 
F 
I 
30.0 
none 
2.0 
30.0 
none
Blanking
OP10 Draw
OP20 Trim
OP30 Flanging
Figure 25-2.  A stamping process consists of draw, trim and flanging (Courtesy
of  Metal  Forming  Analysis  Corporation).    The  labels  OP10,  OP20,  and  OP30  are
used extensively in the ensuing discussion. 
Target Card.  See “Target curves (target.xyz)” in Figure 25-1. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME1 
A80 
none 
Final Blank Card.  See “Final blank (final.k)” in Figure 25-1. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME2 
A80 
none
Initial Blank Card.  See “Initial blank (initial.k)” in Figure 25-1. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME3 
A80 
none 
Reference Surface Card.  See “Reference surface (ref3.k)” in Figure 25-1 and Example II.
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME4 
A80 
none
Reference Surface Card.  See “Reference surface (ref4.k)” in Figure 25-1 and Example II.
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME13 
A80 
none 
Card set for *INTERFACE_BLANKSIZE_INITIAL_TRIM. 
Initial  Flat  Blank.    FILENAME5  should  specify  the  mesh  of  a  blank  that  has  been 
refined  during  a  subsequent  forming  operation.    FILENAME5  is  usually  set  to  the 
adapt.msh output.  See “OP10 Initial Adapted blank mesh” in Figure 25-3. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME5 
A80 
none 
Formed  blank.    FILENAME6  specifies  a  dynain  file  from  a  forming  simulation.    See 
“OP10 Final Blank” in Figure 25-3. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME6 
A80 
none
OP10 initial adapted 
blank mesh (.msh)
OP10 final blank
(adapted)
OP20 final blank
(adapted around hole)
OP20 flat new
(intermediate output)
OP30 Target 
(nearly uniform 
tool mesh)
OP30 flat new
(more mesh around hole, 
intermediate output)
OP30 initial blank
(more mesh around 
hole, .msh file)
OP30 initial blank 
(adapted)
OP30 final blank
(more mesh around hole)
OP10 flat trim 
outline (output))
Figure  25-3.    Inputs  and  outputs  (Courtesy  of  Metal  Forming  Analysis  Corp.).
For exposition of labels OP10, OP20, and OP30 see Figure 25-2. 
Trimmed Formed Blank.  A dynain file from a trimming simulation that started with 
the state given in FILENAME6.  See “OP20 Final Blank” in Figure 25-3. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME7 
A80 
none
Trimmed  Flat  Blank  (output).    This  field  specifies  the  name  for  the  file  to  which  the 
trimmed flat blank is written.  See “OP20 Flat New” in Figure 25-3. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME8 
A80 
none 
Card set for *INTERFACE_BLANKSIZE_INITIAL_ADAPTIVE. 
Flat Blank.  FILENAME9 specifies the mesh of a blank in a flat configuration serving as 
the basis for a two-step metal forming process.  The second-stage simulation produces 
an adapt.msh file, from which the refinements are to be mapped onto the flat-blank of 
FILENAME9.    See,  for  example,  “OP20  Flat  New”  in  Figure  25-3  where  FILENAME9 
points to result, FILENAME8, of an INITIAL_TRIM calculation. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME9 
A80 
none
Initial Blank.  FILENAME10 is the result from the first stage of a two-step process.  See, 
for example, “OP30 Initial Blank” in Figure 25-3 where FILENAME10 has been formed 
and trimmed and refined along the way. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME10 
A80 
none 
Adapted  Initial  Blank.    FILENAME11  contains  a  refined  version  of  the  mesh  in 
FILENAME10.  It is expect to name the adapt.msh file from some operation performed 
on the mesh of FILENAME10.  See, for example, “OP30 Initial Blank (with more mesh)” in 
Figure 25-3, where the adapt.msh file comes from a flanging simulation. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME11 
A80 
none 
Refined  Flat  Blank  (output).    This  field  specifies  the  name  of  the  file  to  which  the 
refined flat blank is written.  The blank’s mesh is refined to exactly match the forming 
process.  See, for example, “OP30 Flat New” in Figure 25-3. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME12 
A80 
none 
Card set for *INTERFACE_BLANKSIZE_SCALE_FACTOR.
Scale  Factor  Card.    Define  one  card  for  each  curve.    Include  as  many  cards  in  the 
following format as desired.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
Variable 
IDCRV 
Type 
Default 
I 
1 
2 
SF 
F 
0.0 
3 
4 
5 
6 
7 
8 
OFFX 
OFFY 
OFFZ 
F 
0 
F 
0 
F 
0 
Card set for *INTERFACE_BLANKSIZE_SYMMETRIC_PLANE. 
Symmetric Plane Card. 
  Card 1 
Variable 
1 
X0 
Type 
F 
2 
Y0 
F 
3 
Z0 
F 
4 
V1 
F 
5 
V2 
F 
6 
V3 
F 
7 
8 
Default 
0.0 
0.0 
0.0 
1.0 
0.0 
0.0
VARIABLE   
DESCRIPTION
IOPTION 
Target curve definition input type: 
EQ.1:  (entire) blank mesh in keyword format. 
EQ.2:  consecutive  position  coordinates  of  blank  boundary
loop  curve  in  XYZ  format,  defined  by  *DEFINE_TAR-
GET_BOUNDARY.    The  blank  mesh’s  normal  vector 
and  the  closed  boundary  curve  are  consistently  orient-
ed  according  to  the  right-hand  rule,  see  Figure  25-4. 
Note  the  target  boundary  curves  must  have  enough
points  for  a  successful  prediction  of  the  initial  blank
size.  Starting in Revision 100589, curve direction is de-
sensitized,  meaning  both  IOPTION = 2  and  IOP-
TION = -2 will give the same results. 
EQ.-2: consecutive  position  coordinates  of  blank  boundary
loop  in  XYZ  format,  defined  by  *DEFINE_TARGET_-
BOUNDARY.  The blank mesh’s normal vector and the
closed  boundary  curve  are  consistently  oriented  ac-
cording to the left-hand rule, see Figure 25-4.  Note the 
target boundary curves must have enough points for a
successful  prediction  of  the  initial  blank  size.    Starting
in  Revision  100589,  curve  direction  is  desensitized, 
meaning  both  IOPTION = 2  and  IOPTION = -2  will 
give the same results. 
In LS-PrePost 4.0, menu option GeoTol → ID Measure can be used 
to  show  the  flow  direction  of  a  boundary  curve.    Curve  →
Rever(se) can be used to reverse the curve direction.
mesh normal direction
mesh normal direction
IOPTION=2
IOPTION=-2
Figure 25-4.  Differences between IOPTION 2 and -2.  Note Starting in 
Revision 100589, curve direction is desensitized, meaning both IOPTION = 2 
and IOPTION = -2 will give the same results. 
  VARIABLE   
IADAPT 
DESCRIPTION
Adaptive mesh control flag.  If IADAPT = 1, number of elements 
between  initial  (FILENAME3)  and  simulated  blank  (FILE-
NAME2) meshes can be different, so it is not necessary to use the
sheet  blank  from  the  file  “adapt.msh”  (created  by  setting 
IOFLAG = 1  in  *CONTROL_ADAPTIVE)  for  the  initial  blank 
mesh. 
MAXSIZE 
The maximum change in initial blank size in each iteration.  It is
used  to  limit  the  blank  size  change  in  each  iteration  during
mapping  to  avoid  convergence  problems  when  the  initial  blank
is curved. 
REFERENC 
Flag  to  indicate  trim  curve  projection  to  a  reference  surface 
(mesh), see Figure 25-1: 
EQ.0: no projection. 
EQ.1: the trim curves will be projected to the reference surface.
In  addition,  the  mesh  file  for  the  reference  surface  is
given in FILENAME4.
VARIABLE   
SPACE 
DESCRIPTION
Point spacing distance on the reference surface for the projected 
curve,  see  Figure  25-1.    If  the  gap  between  two  neighboring 
points  in  the  modified  trimming  curve  is  larger  than  this  value,
extra nodes will be added in the final blank and projected to the 
reference  surface.    Smaller  value  should  be  used  for  large
reference surface curvature. 
MAXGAP 
When  REFERENC  is  set  to  “1”,  the  nodes  from  the  final  blank
will  be  projected  to  the  reference  surface.    However,  if  the
distance  between  the  nodes  and  the  surface  is  larger  than
MAXGAP, the nodes will not be projected. 
ORIENT 
A flag to control iterative optimization efficiency or to include a 
reference surface file for the final formed blank. 
EQ.1: activates  a  new  algorithm  to  potentially  reduce  the
number  of  iterations  during  iterative  blank  size  optimi-
zation  loop,  to  be  used  in  conjunction  with  the  option
SCALE_FACTOR (0.75~0.9). 
EQ.2: to 
(in
include  a  reference  surface  FILENAME13 
keyword  mesh  format)  for  the  simulated  (formed)
blank.  This is useful when formed blank is smaller than
intended and extended surface are not flat.  See Remarks
and Figure 25-1. 
Target  input  file  name.    When  a  blank  mesh  is  used  (IOP-
TION = 1),  the  keyword  file  must  contain  *NODE  and  *ELE-
MENT_SHELL  keywords.    When  using  the  blank  boundary
curve  for  target  (|IOPTION| = 2),  the  file  must  consist  of  *DE-
FINE_TARGET_BOUNDARY.    See  the  Target  Boundaries  (and 
IGES) in the remarks section. 
Simulated  (formed  or  flanged)  sheet  blank  mesh  in  keyword
format.    This  mesh  can  be  obtained  from  the  final  state  of  any 
downstream process simulation. 
Initial sheet blank mesh in keyword format.  This can be the first
state  mesh  from  any  process  simulation  prior  to  FILENAME2
simulation.    Set  IADAPT = 1  if  adaptive  refinement  is  used  in 
any simulation. 
FILENAME1 
FILENAME2 
FILENAME3
VARIABLE   
FILENAME4 
FILENAME5 
FILENAME6 
FILENAME7 
DESCRIPTION
Reference  surface  onto  which  adjustments  to  the  blank’s  trim
curves in its initial state are projected (ref3.k in Figure 25-1).  This 
surface  is  typically  a  curved  extension  of  the  initial  blank  and
must  be  defined  as  mesh  in  keyword  format.    This  file  name
must be defined when REFERENC is set to 1.  Also see extended
reference  surface  for  the  final  state  (formed  state)  -  FILE-
NAME13. 
Initial  blank  in  its  flat  configuration  with  adapted  mesh  in 
keyword  format.    FILENAME5  usually  points  to  an  adapt.msh
file.    For  example  see  OP10  in  Figures  25-2,  25-22  and  25-3,  in 
which  FILENAME5  is  the  adapt.msh  from  a  draw-forming 
calculation. 
Final  formed  blank  in  keyword  format.    This  is  usually  the
dynain file corresponding to the adapt.msh file mentioned above 
for FILENAME5, see Figures 25-2, 25-22 and 25-3. 
A trimmed blank in keyword format.  This file should be derived
from FILENAME6 as the dynain file from a trimming simulation. 
See OP20 in Figures 25-2, 25-22 and 25-3. 
FILENAME8 
This field specifies the name for the file in which the trimmed flat
blank is to be written.  See OP20 in Figures 25-2, 25-22 and 25-3. 
FILENAME9 
FILENAME9 should point to the blank defined by FILENAME8,
as in Figures 25-2, 25-22 and 25-3. 
FILENAME10 
FILENAME11 
Initial-stage result file name.  This may be extracted from d3plot
files  using  LS-PrePost  or  it  may  be  generated  by  LS-DYNA  as  a 
dynain file.  See, for example, “OP30 Initial Blank” in Figure 25-3
where  FILENAME10  has  been  formed,  trimmed  and  refined
along the way. 
To obtain from d3plot file the necessary mesh in keyword format 
using  LS-PrePost4.0  select  POST  →  OUTPUT  →  Dynain  ASCII 
and check the box for “Exclude strain and stress”.  
FILENAME11  contains  a  refined  version  of  the  mesh  in
FILENAME10.    FILENAME11  can  be  obtained  from  adapt.msh
file  from  the  same  operation  performed  on  the  mesh  of
FILENAME10.    See,  for  example,  “OP30  Initial  Blank  (with  more 
mesh)”  in  Figure  25-3,  where  the  adapt.msh  file  comes  from  a 
flanging calculation.
VARIABLE   
FILENAME12 
FILENAME13 
IDCRV 
SF 
OFFX, OFFY, 
OFFZ 
DESCRIPTION
This  field  specifies  the  name  of  the  file  to  which  the  refined  flat
blank is written.  The blank’s mesh is refined to exactly match the 
forming  process.    See,  for  example,  “OP30  Flat  New”  in  Figure 
25-3. 
Reference  surface  onto  which  adjustments  to  the  blank’s  trim
curves in its final state are projected (ref4.k in Figure 25-1).  This 
surface  is  typically  a  curved  extension  of  the  formed  blank  and
must  be  defined  as  mesh  in  keyword  format.    This  file  name
must be defined when ORIENT is set to 2. 
Curve  ID  in  the  order  of  appearance  as  in  FILENAME1  in  the 
target card, as defined by *DEFINE_TARGET_BOUNDARY. 
Scale factor for the IDCRV defined above.  It defines a fraction of
the changes required for the predicted initial blank shape. 
For  example,  if  SF  is  set  to  “0.0”  the  corresponding  IDCRV  will
be  excluded  from  the  calculation  (although  the  original  initial 
curve still will be output); on the other hand, if SF is set to “1.0”,
full  change  will  be  applied  to  obtain  the  modified  initial  blank
that  reflects  the  forming  process.    A  SF  of  0.5  will  apply  50%  of
the  changes  required  to  map  the  initial  blank.    This  feature  is 
especially  important  for  inner  holes  that  are  small  and  hole
boundary  expansions  are  large,  so  the  predicted  initial  hole  can
avoid  “crisscross”  situation.    An  example  is  provided  in  Scale 
Factor and Symmetric Plane. 
Translational  move  of  the  target  curve.    This  is  useful  when
multiple  target  curves  (e.g.    holes)  and  formed  curves  are  far
away  from  each  other.    Input  values  of  OFFX,  OFFY  and  OFFZ
helps  establish  one-to-one  correspondence  between  each  target 
curve and formed curve. 
OFFX.EQ.-10000.0:  offset values are automatically calculated.
X0, Y0, Z0 
V1, V2, V3 
𝑥,  𝑦,  𝑧  coordinates  of  a  point  on  the  symmetric  plane.    See
example in  Scale Factor and Symmetric Plane. 
Vector  components  of  the  symmetric  plane’s  normal.    See
example in  Scale Factor and Symmetric Plane.
Compulational 
Cost 
Accuracy 
Information 
Required 
Physical 
Process 
Blanksize  Full simulation 
Exact 
Full Simulation 
Any 
Unflanging  Fast 
Approximate 
Process Geometry 
Inverse Flanging 
Onestep  Fast 
Approximate 
None 
(Path independent) 
Any 
Table 25-1.  Comparison of inverse methods. 
Inverse Methods for Optimizing Blank Size and Trim Lines: 
Finding the minimal practicable blank size and developing an optimal set of trim lines 
is  an  integral  part  of  the  die  engineering  process.    This  card,  *INTERFACE_BLANK-
SIZE, is one of several features that have been developed to solve the inverse problem: 
that is to calculate an initial blank or blank boundary that will yield a desired product 
based mostly on the target geometry of that final product. 
1.  The  One-Step  Method.    The  *CONTROL_FORMING_ONESTEP  card  is 
suitable for early blank-size estimates.  It invokes the total-strain theory of plas-
ticity  thereby  bypassing  the,  as  of  yet,  undetermined  specific  details  of  the 
forming process. 
2.  Unflanging.    Once  product  design  and  process  plan  are  complete,  die 
development begins with addendum and binder creation, followed by second-
ary  tooling  development.    In  this  stage,  *CONTROL_FORMING_UNFLANG-
ING  can  be  used  to  develop  trim  lines  for  the  secondary  tooling;  final  (or 
intermediate) desired flange shapes are unfolded onto the addendum or binder 
to  obtain  the  corresponding  flange  shapes  in  its  initial  shape.    It  also  imple-
ments failure criteria to arrive at suggested final flange curves, with strains and 
thickness output on the unfolded flanges. 
3. 
Interface  Blanksize.    This  card,  *INTERFACE_BLANKSIZE,  can  be  used  to 
accurately  determine  the  optimal  initial  blank.    To  do  so  it  requires  on  initial 
configuration, the corresponding simulated configuration, and a desired target 
configuration.    This  method  takes  into  account  the  entire  metal-forming  pro-
cess. 
a)  One  application  of  this  keyword  is  to  map  trim  curves  between  dies  to 
calculate the trim curves needed for all trim dies.  An example of the ap-
plication can be found in Figures 25-18 through 25-21.
Draw(flanging) 
simulation
Initial blank
Final blank
Target blank/boundary
Reference surface
*INTERFACE_BLANKSIZE
_[OPTION]
Final blank size 
within tolerance of
the target blank?
Yes
Done
DOS or linux 
commands
No
Figure 25-5.  An iterative blank size development process. 
b)  The  keyword  can  also  be  used  to  determine  the  precise  minimal  initial 
blank needed for a draw panel whose blank edge must be at specified dis-
tances from the edge of the draw beads. 
Iterative Workflow: 
The  “interface  blanksize”  command  produces  an adjusted  initial  blank.    It  is  not  to  be 
expected that the adjustment will be exact.  However, this initial blank shape can be run 
through a second simulation to see if the final shape is close enough to the target blank.  
If  it  is  not  close  enough,  then  the  results  from  the  second  simulation  can  be  used  to 
repeat the process.  Iterations can proceed until the final shape is within the range of the 
target shape.  This iterative blank size development process is schematically presented 
in Figure 25-5 and exemplified in Figures 25-8 through 25-17. 
Target Boundaries (and IGES): 
When  IOPTION = 2,  or  -2,  a  file  with  the  keyword  *DEFINE_TARGET_BOUNDARY 
must  be  present.    This  keyword  can  now  be  created  from  an  IGES  file  using  LS-
PrePost4.1  (or  4.2).    To  convert  from  IGES  curves  to  keyword  *DEFINE_TARGET_-
BOUNDARY in LS-PrePost4.1, use menu option Curve → Convert→ Method (To Keyword) 
→ Select *DEFINE_TARGET_BOUNDARY; pick the curves then hit “To Key”; write out 
the keyword file using File → Save as → Save Keyword As, and select “Output Version” 
as  “V971_R7”.    In  LS-PrePost 4.2,  a  GUI  interface  was  developed  located  at  Applica-
tion/Metal Forming/Blanksize Trimline so users can import the target curve directly in 
IGES format, the initial and final blank mesh and then write out a complete LS-DYNA 
input deck.
In addition, the target curves should be projected onto the final blank mesh if they do 
not exactly lie on the mesh surface.  This can be done with LS-PrePost4.1 via the menu 
option GeoTol → Project → Project, select Closest Projection, select Project to Elements, then 
define  the  destination  mesh  and  source  curves,  and  hit  Apply.    3-D  projection  in  LS-
PrePost4.2  can  be  critical  in  obtaining  a  perfectly  smooth  predicted  initial  boundary 
curve  trimcurves.ibo  after  the  LS-DYNA run.    Note  the  projected target  curves  should 
be used to import into the GUI. 
Computed Initial Blank Boundaries (and IGES): 
Computed  boundary  curves  are  written  with  *DEFINE_CURVE_TRIM_3D  keyword 
into  a  file  called  trimcurves.ibo.    The  format  of  this  file  follows  the  keyword’s 
specification.  LS-PrePost4.0 can convert the computed curve to IGES.  See Figure 25-10.  
After hitting Apply, the curves will show up in the graphics window, and File → Save as 
→ Save Geom as can be used to write the curves out in IGES format.  In the LS-PrePost4.2 
GUI,  under  Results,  trimcurves.ibo  can  be  directly  imported  into  the  graphics  window 
for viewing and to save in either STEP or IGES format. 
To convert IGES to the *DEFINE_CURVE_TRIM_3D keyword format import the IGES 
file into LS-PrePost4.0, and follow the procedures shown in Figure 25-11.  After finishing 
step  2,  “curves  have  been  converted  to  keyword  format”  will  be  reported  in  the  command 
prompt.  Then use File → Save → Save keyword to write out the keyword file. 
Support for Multi-Stage Processes with the Development Option: 
Original Implementation. 
Prior  to  Revision  88708  the  development  option  required  that  the  final  blank 
(FILENAME2)  differ  from  the  initial  blank  (FILENAME3)  by  no  more  than  a 
deformation  and  mesh  refinement.    In  practice,  this  means  that  the  two  meshes  must 
come  from  the  same  process  simulation.    For  example,  in  a  draw,  trim  and  flanging 
process,  the  trimmed  panel  mesh  is  used  for  flanging  simulation.   Therefore,  with  the 
original  implementation,  LS-DYNA  required  that  the  initial  blank  state  (FILENAME3) 
be  trimmed  when  the  final  blank  state  (FILENAME2)  is  flanged  on  trimmed  panel.  
Failure to observe this limitation may result in error termination.
Output: predicted initial 
blank outline (station 1)
Input: initial blank 
shape (station 1)
Input: target part boundary 
outline (station 2)
Input: simulated blank 
final shape (station 2)
Figure 25-6.  Blank size development in a progressive die with IADAPT = 1 in 
Example I 
Enhanced Implementation. 
A  more  recent  improvement  to  the  blank  size  development  (Revision  88708)  removes 
the requirement that initial (FILENAME3) and final (FILENAME2) blanks must be from 
the  same  process  simulations.    The  initial  and  final  blank  states  may  differ  by  a 
trimming  process.    This  allows  trimming  and  other  process  such  as  flanging  to  occur 
between  the  initial  and  final  blanks,  without  the  need  of  invoking  the  INITIAL_TRIM 
and INITIAL_ADAPTIVE options.  For example, the initial blank can be the blank mesh 
from  “Blanking”  in  Figure  25-2,  and  the  final  blank  can  be  the  blank  mesh  from 
“Flanging,” which is also in Figure 25-2. 
Scale Factor and Symmetric Plane: 
An example of using various scale factors ranging from 0.0 to 1.0 on a model involving 
an initial hole shape is shown in Figure 25-25.  The target curve is given in targetline.k.  
All  nodes  along  the  symmetric  plane  are  constrained  by  the  SYMMETRIC_PLANE 
option.  The symmetric plane is defined going through point coordinates (-76, 2.63844, 
0.38) with plane normal vector of (1.0, 0.0, 0.0).  A complete input is provided below: 
*KEYWORD 
*INTERFACE_BLANKSIZE_DEVELOPMENT 
$  IOPTION              IADAPT 
        -2                   1 
$ target boundary curves 
targetline.k 
$ final formed mesh 
final.k 
$ initial mesh
initial.k 
*INTERFACE_BLANKSIZE_SCALE_FACTOR 
$    IDCRV        SF 
         1       0.2 
*INTERFACE_BLANKSIZE_SYMMETRIC_PLANE 
$       X0        Y0        Z0        V1        V2        V3 
       -76   2.63844      0.38       1.0       0.0       0.0 
*END 
If taregetline.k consists of multiple curves, the following format can be used: 
*INTERFACE_BLANKSIZE_SCALE_FACTOR 
$    IDCRV        SF 
         1       0.2 
         2       0.8 
         3       1.0 
                ⋮                 ⋮ 
Example I: Simple Example of the Development Option 
Given the initial and final blank configuration and a target, this option calculates a new 
initial blank outline, corresponding to the target final blank boundary.  In this example 
note  that  IADAPT = 1,  meaning  initial  and  final  blank  meshes  may  differ  by  an 
adaptively operation.  The input and output files are detailed below, and output results 
are shown in Figure 25-6. 
*KEYWORD 
*INTERFACE_BLANKSIZE_DEVELOPMENT 
$  IOPTION              IADAPT 
         2                   1 
$  input file for target mesh, or target position coordinates 
targetpoints.k 
$  input file for formed mesh 
final.k 
$  input file for initial blank mesh 
initial.k 
*END 
The  file,  targetpoints.k,  is  partially  shown  below  was  generated  from  IGES  using  LS-
PrePost 4.1. 
*KEYWORD 
*DEFINE_TARGET_BOUNDARY 
    -1.83355e+02    -5.94068e+02    -1.58639e+02 
    -1.80736e+02    -5.94071e+02    -1.58196e+02 
    -1.78126e+02    -5.94098e+02    -1.57813e+02 
    -1.75546e+02    -5.94096e+02    -1.57433e+02 
    -1.72888e+02    -5.94117e+02    -1.57026e+02 
          ⋮                ⋮               ⋮ 
    -1.83355e+02    -5.94068e+02    -1.58639e+02 
*END 
The output is the modified initial blank outline in the file trimcurves.ibo.
Example II: The Reference Surface feature for the Development Option 
For an initial blank that is not flat, the fields REFERENC and FILENAME4 can be used 
to define a surface onto which changes in the boundary are needed.  This is important 
when the adjusted boundary is not a simple tangential extension of the initial blank. 
In  a  keyword  example  below,  REFERENC  is  set  to  “1”  and  the  reference  file  for  the 
extended initial shape is given as ref3.k.  The maximum change between the initial and 
final  blank  size  is  set  to  be  20.0  mm  per  iteration.    Point  spacing  distance  (SPACE)  of 
calculated trim curve on the reference surface is set at 2.0 mm.  Note that the inner holes 
and  outer  boundary  curves  are  defined  in  “target.xyz”.    The  holes  do  not  necessarily 
need  to  exist  in  the  initial  or  final  blank  mesh.    Also,  since  ORIENT  is  set  to  “2”,  a 
reference  surface  mesh  file  (ref4.k)  is  provided  for  the  final  (formed)  state.    The  input 
details and output results are shown in Figure 25-1. 
*KEYWORD 
*INTERFACE_BLANKSIZE_DEVELOPMENT 
$        1         2         3         4         5         6         7         8 
$  IOPTION              IADAPT   MAXSIZE REFERENCE     SPACE              ORIENT 
        -2                   1    20.000         1       2.0                   2 
$  input file for target mesh: 
target.xyz 
$  input file for formed mesh: 
final.k 
$  input file for initial blank mesh: 
initial.k 
$  reference file for extended initial shape: 
ref3.k 
$  reference file for extended final shape: 
Ref4.k 
*END
Blank edge 10mm outside
of last draw bead bend
Cross Member in Air Draw
Target Blank Edges 10 mm Outside of Beads
Figure 25-7.  NUMISHEET 2005 cross member in Exmaple III. 
Example III: Development Feature Applied to a Draw Die with Physical Bead 
In  this  example,  which  was  created  from  NUMISHEET  2005,  the  DEVELOPMENT 
option has been used to design a blank such that, when formed, the edge is a specified 
distance outside of the last bend of a draw bead.  In Figure 25-7, the tooling and blank 
set up is shown to the left.  The right side of the figure shows the target blank, whose 
left  and  right  edges  everywhere  are  made  10mm  outside  of  the  last  bending  radius  of 
the draw beads.  This  setup is prototypical of one method to ensure a very stable and 
high-quality stamping process. 
The first step towards setting up this analysis was to use *CONTROL_FORMING_ON-
ESTEP to unfold the target blank and thereby obtain an initial guess of a flat blank, as 
shown to the left if Figure 25-12.  The flat blank is then formed as one would usually do 
in  a  regular  forming  simulation,  shown  on  the  right  side  of  the  figure.    The  formed 
blank (Iteration 0) turns out to be larger than the target. 
Next, the DEVELOPMENT is applied to generate a new and better initial blank that will 
lead to the target blank.  The flat blank is used as input for the “initial blank mesh”, the 
formed blank is used as input for the “simulated mesh”, and the target blank mesh, or 
boundary points is used to define the target. 
In  Figure  25-13  (left)  the  improved  initial  blank,  called  the  first  compensated  blank,  is 
superimposed onto the original one-step unfolded result.  The one-step unfolded result 
is  somewhat  larger  than  the  developed  blank.    When  formed  the  improved  blank 
(Iteration 1) nearly overlaps the target blank, shown in Figure 25-13 (right).  If the final 
formed  blank  still  deviates  from  the  target,  another  iteration  would  ensue,  until 
satisfactory results are obtained.
Gravity loaded 
Binder surface
Figure 25-8.  NUMISHEET 2008 B-pillar; Gravity loaded blank. 
Lower punch
Example IV: Iterating with the Development Option 
Because the NUMISHEET 2008 B-pillar model involves neither trimming nor flanging, 
it  exmplifies  the  DEVELOPMENT  option  in  its  most  direct  use  case.    This  model, 
illustrated in Figure 25-8, simulates a draw-die’s action on a gravity-stressed flat blank.  
The B-pillar undergoes a stamping process including gravity, binder closing, and being 
drawn.  In this example the DEVELOPMENT option is used to calculate the geometry 
for  an  initial  blank  that  will    exactly  satisfy  the  design  specification  for  a  final  formed 
panel.    To  highlight  the  efficiency  of  this  feature,  we  start  with  an  initial  blank  whose 
formed product deviates from the specification by a wide margin and then iterate using 
the DEVELOPMENT feature. 
The target and the optimal initial blank are shown in Figure 25-14.  The intial guess is 
intentionally  deviated  from  the  optimal  initial  blank  as  shown  in  the  left  panel  of 
Figure 25-15; while the formed blank is compared with the target in the right panel. 
In the first iteration a new initial blank is computed, and illustrated in the left panel of 
Figure 25-16  bearing  the  label,  1st  compensated  blank.    The  simulation  is  repeated  using 
the first compensated blank, and in the right panel the result is compared to the target.  
The formed blank is narrower in the notched areas as compared with the target. 
The  second  iterate  is  shown  in  the  left  panel  of  Figure  25-17  bearing  the  label,  2nd 
compensated  blank.    Again,  the  simulation  is  repeated,  but  this  time  using  the  second 
compenated  blank,  and  the  result  is  compared  to  the  target  in  the  right  panel  of 
Figure 25-17.  The resulting product is a good match to the target. 
Because  of  the  initial  blank  was  intentionally  deviated  from  its  ideal  shape  by  a  large 
margin,  this  example  requires  two  iterations  to  converge.    Generally  this  processed  is 
bootstrapped  with  the  *CONTROL_FORMING_ONESTEP  card,  which  calculates  an 
initial guess by approximately unfolding the target shape.
Forming
Trimming
Blanking (OP10 
initial blank)
OP10 
OP20 
Forming
Bending
Flanging
OP30 
OP40 
OP50 
Courtesy of T&D Design, LLC, U.S.A
Flanging
Figure  25-9.   Enhanced  DEVELOPMENT feature on a progressive die.   Even
though  trimming  occurs  at  OP20  the  algorithm  requires  as  input  only  OP10,
OP50, and a target  geometry. 
Example V: Development Feature Applied to Flanging Process 
In  this  example,  which  is  schematically  illustrated  in  Figure 25-18,  the  NUMISHEET 
2002 fender outer is flanged along the hood line.  The development feature adjusts the 
initial  blank’s  boundary  so  that  the  formed  piece  matches  the  specified  target  flanged 
shape as shown in Figure 25-19.  For demonstration purposes, the trimmed blank shape 
is intentionally deviated from the optimal configuration by a large amount.  This error 
is  indicated  in  Figure  25-20  by  the  label  initial  guess  trim  curves.    In  Figure  25-20  The 
flanged  product  is  shown  to  deviate  substantial  from  the  flanged  target  along  the 
boundary.    As  shown  in  Figure  25-21  after  one  iteration  the  correct  initial  blank 
boundary is obtained.
Alternatively, *CONTROL_FORMING_UNFLANGING can be used to unfold the 
flanged target onto the addendum to obtain the initial blank size, or a starting guess for 
this process. 
Example VI: Enhanced-Development Feature Applied to Progressive Die Process 
In the example of Figure 25-9, courtesy of T&D Design, LLC, U.S.A, the blank-shape for a 
five  stage  progressive  die  process  is  calculated.    Because  this  process  involves  a 
trimming  step,  the  development  capability  prior  to  Revission  88708  does  not  support 
this example. 
In this example, an initial blank at OP10, undergoes trimming, reforming, bending and 
flanging  to  arrive  at  the  blank  in  OP50.    In  figure  25-23  the  computed  product  is 
compared with the specified target.  A blank size development calculation produces the 
modified  OP10  initial  blank  outline.    The  updated  blank  is  used  in  a  verification 
simulation.    As  seen  in  Figure  25-24  the  blank  size  development  feature  produces  a 
good result. 
Trim  lines  are  not  optimized  by  the  development  feature,  so  trimming  should  only 
occur along the boundary of the target blank.  The modified OP10 blank requires some 
refitting in the trimmed area. 
Revision information: 
This feature is available in both SMP and MPP, in double precision only.  Note a GUI 
for using this feature is now available in LS-PrePost as of version 4.2.  It can be accessed 
under APPLICATION → Metal Forming → Blank Size/Trim line Dev.  Starting revision 
information for each feature is listed as follows: 
1.  DEVELOPMENT option: Revision 74605. 
2. 
3. 
INITIAL_TRIM and INITIAL_ADAPTIVE: Revision 75023. 
IADAPT: Revision 75827. 
4.  Command line option “JOBID=…”: Revision 82861. 
5.  MAXSIZE: Revision 85633. 
6.  SPACE: Revision 85755. 
7.  MAXGAP: Revision 85792. 
8.  Reference surface (parameter REFERENC): Revision 86086.
9.  Removal  of  the  restriction  requiring  the  initial  (FILENAME3)  and  the  final 
(FILENAME2)  blanks  must  be  from  the  same  process  simulation:  Revision 
88708. 
10.  Improve smoothness of the output trim curve trimcurves.ibo in case the given 
meshes have warpage caused by wrinkles during forming: Revision 96164. 
11.  Symmetric plane: Revision 97443. 
12.  Scale factor: Revision 98122. 
13.  ORIENT = 1: Revision 100453. 
14.  ORIENT = 2: Revision: 104168. 
15.  Curve direction is desensitized, meaning both IOPTION = 2 and IOPTION = -2 
will give the same results: Revision 100589. 
16.  OFFX, OFFY, OFFZ: Revision 100660. 
17.  Automatically calculate offset values (OFFX.EQ.-10000.0): Revision 102609.
SelPart
RefGeo
Keyword Manage
Keyword Edit   Keyword Search
Keyword
Curve
CreEnt
Surf
PartID
Solid
Display
GeoTol
RefChk
Mesh
Renum
Model
Section
EleTol
MSelect
Post
Subsys
MFPre
Groups
MFPost
Views
Favor1
PtColor
Edit:  DEFINE_CURVE_TRIM_3D                            Edit
                                                  Model       All                 RefBy
3 (right click)
Name                                                                                Count
     DEFINE                                                                          1
           CURVE_TRIM_3D                                                 1
     KEYWORD                                                                    1
           KEYWORD                                                              1
     TITLE                                                                              1
     Delete all     
     Delete by ids
     Transfer to
     Transfer to Curve
Material arrange
GroupBy                         Sort                         List
Model                              Type                        All
Load From MatDB
Model Check
ExpandAll
Keyword Del
  CollapseAll
Done
Transfer to Curve
DEFINE_CURVE_TRIM_3D(1)
From                  1    To
   All               None           Reverse
Apply                    Done
Figure 25-10.  Converting trimcurves.ibo to IGES format in LSPP4.0. 
1 (right click)
   Assembly 1
       Shape Group
           BSpline Edge 1:   
    Curve
       Geom Parts
(un)Blank
Reverse Blank
Delete
Rename
Color
Transparent
Locate
Locate by ID...
Statistical
To 2.x
To Keyword Curve Trim 
3D
Sort by ID
Sort by Type
Figure 25-11.  Converting IGES file to *DEFINE_CURVE_TRIM_3D.
One-step unfold result with 
*CONTROL_FORMING_ONESTEP
Iteration 0: formed from one-step 
unfolded blank
Drawn blank 10mm outside
 of draw beads - Target
Target
Figure 25-12.  Initial blank calculation and baseline formed blank. 
1st compensated blank
using this keyword
Iteration 1: Formed from
1st compensated blank
Original one-step unfold result
Target
  Figure 25-13.  The first compensated blank and the final confirmation run.
Target blank
Target blank 
formed
Figure 25-14.  Assumed target blanks. 
Target blank
Initial guess
Formed from 
initial guess
Target blank 
formed
Figure 25-15.  Iteration 0 results comparison with target.
Target blank
1st compensated blank
Formed from 1st 
compensated blank
Target blank 
formed
Figure 25-16.  Iteration 1 results. 
Target blank
2nd compensated blank
Formed from 2nd 
compensated blank
Target blank 
formed
Figure 25-17.  Iteration 2 results. 
Lower post
Flanging 
steel move
Figure 25-18.  The flanging process on NUMISHEET 2002 fender outer. 
Drawn and trimmed 
Pressure pad
*INTERFACE_BLANKSIZE 
Addendum / binder surface where 
trim lines to be developed
Target part 
(flanged part) 
Drawn panel to be 
trimmed for flanging 
Figure  25-19.   Multiple section view  showing the target  part and addendum
surfaces. 
Flanged shape based on initial guess trim 
curves, deviates from flanged target
Initial guess trim curves 
intentionally off by a large margin
Flanged target
Figure 25-20.  Initial trim curves intentionally made to be off by a large 
margin.
Compensated trim curves
Initial guess
Compensated flanged part
overlaps flanged target 
Figure 25-21.  Compensated trim curves overlap with the target curves.
OP10 final blank
OP20 file name 
for calculated 
initial flat blank 
OP30 adapted 
initial blank mesh 
OP30 file name for 
calculated initial 
flat blank 
OP30 final blank
OP10 initial 
adapted flat blank
OP20 trimmed 
blank
OP30 initial mesh (from 
OP30 d3plots of first state 
with adaptive constraints)
*KEYWORD
*INTERFACE_BLANKSIZE_INITIAL_TRIM
case10.adapt.msh
case10.dynain
case20.dynain
op20_flat_new
*INTERFACE_BLANKSIZE_INITIAL_ADAPTIVE
op20_flat_new
case30start.k
case30.adapt.msh
op30_flat_new
*INTERFACE_BLANKSIZE_DEVELOPMENT
$    IOPTION
                  1
target.k
case30.dynain
op30_flat_new
*END
OP30 target
OP30 initial flat 
blank
User inputs 
LS-DYNA intermediate output files
LS-DYNA simulation output: new trim line OP10 (file "trimcurves.ibo")
Figure 25-22.  File structures for a multi-process blank development.
Input #3: OP10 
initial blank
Input #2: OP50 
formed blank
Output: modified 
OP10 initial blank 
outline
Blanking
Courtesy of T&D Design, LLC, U.S.A
Input #1: OP50 
target boundary
OP50 
  Figure 25-23.  Inputs and output for the enhanced DEVELOPMENT feature.
OP50 formed 
blank outline
Input #1: OP50 
target boundary
OP50 formed blank 
outline coincides with 
the target boundary
Final OP50 formed blank is off 
target in areas indicated
Courtesy of T&D Design, LLC, U.S.A
Final OP50 formed blank meets target 
requirement with OP10 modified blank outline
Figure 25-24.  Verification simulation on a progressive die process.
Initial blank (input)
Final blank 
(input)
Option SYMMETIC 
_PLANE applied on 
nodes along the 
symmetric plane (input)
Output for scale factor: 1.0, or, without 
using option SCALE_FACTOR
Output for scale Factor: 0.2
Final hole 
boundary (input)
Output for scale factor: 0.0, or, 
original initial hole boundary.
Target hole boundary (input)
Figure 25-25.  Options SCALE_FACTOR and SYMMETRIC_PLANE.
*INTERFACE_COMPENSATION_NEW_{OPTION} 
Available options include: 
<BLANK> 
ACCELERATOR 
MULTI_STEPS 
LOCAL_SMOOTH 
PART_CHANGE 
REFINE_RIGID 
Purpose:    This  card  encompasses  several  methods  for  spring  back  compensation  in 
stamping  tools.    The  applications  for  this  card  include:  (1)  calculating  the  deviation  of 
the stamped part from its intended design, and to automatically compensate the tool to 
minimize the deviation; (2) to map the existing trim curve to the modified tool; and (3) 
to automatically detect undercut. 
This keyword employs a nonlinear iterative method.  Usually, it takes between 2 and 4 
iterations  to  converge  within  tolerances.    Additionally,  this  method  provides  a  scale 
factor,  which  allows  the  user  to  decide  the  ratio  of  shape  deviation  the  part  is 
compensated. 
Options 
The  ACCELERATOR  option  speeds  up  the  convergence  rate  in  reducing  the  part 
deviation to design tolerance thus reducing the number of iterations.  This option also 
allows for a much simpler user interface. 
The  MULTI_STEPS  option  allows  for  tooling  compensation  of  the  next  die  process, 
based  on  target  blank  shape,  compensated  blank  shape  for  the  next  step,  and  current 
tools.  This feature is useful in line die process/tooling compensation. 
The  LOCAL_SMOOTH  option  features  smoothing  of  a  tool’s  local  area  mesh,  which 
could become distorted because of either bad or coarse mesh of the original tool surface, 
or  in  areas  where  tooling  pairs  (for  example,  flanging  post  and  flanging  steel)  do  not 
maintain a constant gap, or after a few compensation iterations. 
The  PART_CHANGE  option  allows  for  updating  of  the  final  compensated  tool  using 
the changed part or formed blank shape, thus eliminating the need for going through a 
new compensation iteration loop.  This option is used together with *INCLUDE_COM-
PENSATION_UPDATED_BLANK_SHAPE,  and  *INCLUDE_COMPENSATION_UP-
DATED_RIGID_TOOL.
The  REFINE_RIGID  option  refines  the  rigid  tool  mesh  based  on  user-provided  trim 
curves.  It also realigns the mesh so no elements cross the trim curves.  This feature only 
needs  to  be  done  once  before  the  iterative  springback  compensation  begins.    The 
modified rigid too mesh will greatly improve the convergence in the iterative process. 
Known Limitation 
The current methods sometimes fail to eliminate undercut. 
All required input files must be included by using various options in the keyword: *IN-
CLUDE_COMPENSATION_{OPTION}.    The  option  LOCAL_SMOOTH  also  needs  to 
use a keyword *SET_NODE_LIST_SMOOTH. 
Card 1 for <BLANK>, MULTI-STEPS, and LOCAL_SMOOTH options. 
  Card 1 
1 
Variable  METHOD 
Type 
Default 
I 
6 
2 
SL 
F 
3 
SF 
F 
5.0 
0.75 
4 
5 
6 
7 
8 
ELREF 
PSIDM 
UNDCT 
ANGLE 
NLINEAR 
I 
1 
F 
F 
F 
none 
none 
0.0 
I 
1 
Card 1 for keyword ACCELERATOR option. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ISTEPS 
TOLX 
TOLY 
TOLZ 
OPTION 
Type 
Default 
I 
0 
F 
F 
F 
0.5 
0.5 
0.5 
I
Card 1 for keyword option PART_CHANGE: 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MAXGAP 
Type 
F 
Default 
none 
Card 1 for keyword option REFINE_RIGID: 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME1 
A80 
none 
Card 2 for keyword option REFINE_RIGID: 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
  VARIABLE   
METHOD 
SL 
FILENAME2 
A80 
none 
DESCRIPTION
There  are  several  extrapolation  methods  for  the  addendum  and
binder outside of trim lines, see Remarks. 
The  smooth  level  parameter  controls  the  smoothness  of  the
modified  surfaces.    A  large  value  makes  the  surface  smoother.
Typically  the  value  ranges  from  5  to  10.    If  spring  back  is  large,
the transition region is expected to be large.  However, by using a
smaller value of SL, the region of transition can be reduced.
VARIABLE   
DESCRIPTION
SF 
Shape  compensation  scale  factor.    The  value  scales  the  spring
back  amount  of  the  blank  and  the  scaled  amount  is  used  to
compensate the tooling. 
GT.0: compensate in the opposite direction of the spring back; 
LT.0:  compensate 
in 
the  punch  moving  direction 
(for
undercut). 
This  scale  factor  scales  how  much  of  the  shape  deviation  is
compensated.  For example, if 10 mm of spring back is predicted,
and  the  scale  factor  is  chosen  as  0.75,  then  the  compensation  in 
the opposite direction will only be 7.5 mm. 
Experience  shows  that  the  best  scale  factor  for  reaching  a
converged solution (within part tolerance) is case dependent.  In
some  cases,  a  scale  factor  range  of  0.5  to  0.75  is  best;  while  in
others, larger values are indicated.  Sometimes, the best value can 
be  larger  than  1.1.    Note  that  within  an  automatic  compensation
loop, this factor does not need to be varied. 
Since it is impossible to choose the best value for each application
up front 0.75 is recommended for the first attempt.  If the spring
back  cannot  be  effectively  compensated  and  the  calculation
diverges, the factor can be moved upward or downward to obtain
a  converged  solution,  or  more  iterations  must  be  used  with  the
initial trial value to compensate the remaining shape deviation. 
For  channel  shaped  parts  that  have  a  twisting  mode  of  spring
back, the scale factor is more important.  It was found that a small
change of the tool shape might change the twisting mode.  If this
occurs, using a small value (<0.5) is suggested. 
ELREF 
Element refinement option: 
EQ.1: special element refinement is used with the tool elements
(default); 
EQ.2: special element refinement is turned off.
VARIABLE   
PSIDM 
DESCRIPTION
Define the part set ID for master parts.  It is important to properly
choose  the  parts  for  the  master  side.    Usually,  only  one  side 
(master side) of the tool will be chosen as the master side, and the
modifications  made  to  the  other  side  (slave  side)  depends  solely
on  the  changes  in  the  master.    This  allows  the  two  sides  to  be
coupled  and  a  constant  (tool)  gap  between  the  two  sides  is 
maintained.    If  both  sides  are  chosen  to  be  master,  the  gap
between  the  two  sides  might  change  and  become  inhomogene-
ous. 
The choice of master side will have an effect on the final result for
method 7 when applied to three-piece draw models.  At this time, 
when  the  punch  and  binder  are  chosen  as  the  master  side,  the
binder  region  will  not  be  changed.    Otherwise,  when  the  die  is
chosen  as  master  side  the  binder  will  be  changed,  since  the
changes extend to the edges of the master tool. 
UNDCT 
Tool undercut treatment option: 
EQ.0: no check (default); 
EQ.1: check and fix undercut. 
ANGLE 
An angle defining the undercut. 
NLINEAR 
Activate nonlinear extrapolation. 
ISTEPS 
Steps in accelerated compensation procedure, see Remarks. 
TOLX 
TOLY 
TOLZ 
Part  deviation  tolerance  between  current  blank  and  target  blank
shape in global 𝑥-direction. 
Part  deviation  tolerance  between  current  blank  and  target  blank
shape in global 𝑦-direction. 
Part  deviation  tolerance  between  current  blank  and  target  blank
shape in global 𝑧-direction. 
OPTION 
Compensation acceleration method.  Currently available only for
method 1. 
MAXGAP 
Maximum gap between the original part and changed part.
VARIABLE   
FILENAME1 
FILENAME2 
DESCRIPTION
Rigid  tool  mesh  file  in  keyword  format.    This  should  be  the
tooling  mesh  used  in  the  forming  or  flanging  simulation,  before
any compensation is done.  The refined rigid tool mesh will be in
the  file  rigid_refined.tmp.    See  Option  REFINE_RIGID:  rigid  tool 
mesh refinement for a better convergence. 
Trim  curves  in  keyword  format  *DEFINE_CURVE_TRIM_3D.
The curves will be used to refine and realign the FILENAME1 to
improve  the  convergence  in  the  iterative  compensation  process. 
The  refined  rigid  tool  mesh  will  be  in  the  file  rigid_refined.tmp. 
See  Option  REFINE_RIGID:  rigid  tool  mesh  refinement  for  a
better convergence. 
Compensation Methods Overview: 
After  trimming,  only  a  limited  part  of  the  tool  has  direct  relationship  with  the  spring 
back  of  the  blank  part.    Modifications  of  the  rigid  tool  outside  the  trimmed  region 
involves extrapolation.  Unfortunately, extrapolating is unstable and tends to generate 
non-smooth  surfaces.    To  resolve  this  problem,  seven  smoothing  algorithms  are 
implemented.    The  most  frequently  used  methods  are  methods  7,  8  and  -8,  while  the 
others are used only occasionally. 
Method 7 
If the punch is chosen as the master side, the binder will not be changed.  Aside from 
the region inside the punch opening the rest of the model is untouched.  Smoothing has 
little  effect  on  method  7.    The  smoothness  of  the  modified  tool  depends  on  the 
magnitude  of  the  spring  back  and  the  size  of  the  addendum  region.    This  method  is 
nonlinearly and, therefore, necessitates an iterative solve. 
Advantages: The binder will not be changed. 
Disadvantages:  The  change  will  be  limited  inside  the  addendum  region,  and  the 
modified  surface  may  not  be  smooth  if  the  spring  back  magnitude  is  large  and  the 
transition is small. 
Method 6 
The  smoothness  and  the  transition  region  of  the  modified  surface  will  depend  on  the 
spring back magnitude and the smoothing factor.  If the spring back magnitude is large, 
the transition region will be increased automatically.  On the other hand, the transition 
region will be smaller if the spring back magnitude is small.  At the same time, a larger
smoothing  factor  will  result  in  a  smaller  transition  region.    Like  method  7,  this  too  is 
nonlinear. 
Advantages: The smoothness of the modified surfaces can be controlled. 
Disadvantages: It is impossible to limit the transition region, and the binder surface (and 
therefore, draw beads) could change if the spring back is large. 
Method 3 
Similar to Method 6, however, it is a linear method and no iteration is necessary. 
Method 8 
This  is  an  enhanced  version  of  Method  6,  and  can  account  for  addendum  and  binder 
changes.    Usually  the  upper  tooling  including  addendum  and  binder  (in  an  air  draw) 
are included in the PSIDM definition. 
Method -8 
This  method is a modification of Method 8,  and is  used for trim die nesting (from the 
drawn panel shape). 
Methods 1, 2, 4, and 5 
These  methods  are  deprecated  and  may  be  removed  in  the  future.    They  are  included 
only for maintaining backwards compatibility.
*PARAMETER
*CONTROL_FORMING_AUTOPOSITION_PARAMETER
*PARAMETER_EXPRESSION
*PART_MOVE
DOS or 
linux commands
Gravity
forming
Trimming
Springback
springback amount 
< tolerance, or, 
iterations = 4?
Yes
Done
No
Compensation
Figure 25-26.  Iterative compensation flow chart 
Preventing Undercut 
When the draw wall is steep, it is likely that undercut will occur.  Since undercut is not 
acceptable in real world die manufacturing, it must be prevented. 
The  compensation  code  can  automatically  detect  undercut  and  issue  a  warning 
message.  Additionally, LS-DYNA will write a list of undercut elements to a file called 
blankundercut.tmp  so  that  the  user  can  easily  identify  which  elements  may  be 
problematic. 
If  the  undercut  is  limited  to  only  a  few  elements,  it  is  possible  to  fix  the  problem 
manually. 
Undercut  can  be  reduced  by  compensating  the  spring  back  only  in  the  punch  moving 
direction (by using a negative scale factor).  This method is not 100% reliable and more 
robust solutions are being studied. 
Iterative spring back compensation 
Figure 25-26 is a flow chart showing the iterative spring back compensation algorithm 
as applied to a typical stamping process.  The first stamping process simulation is done 
following  gravity→forming→trimming→spring  back  (ITERATION  0).    The  stamping 
process  simulation  is  set  up  using  eZ-Setup  (http://ftp.lstc.com/anonymous/out-
going/lsprepost/4.0/metalforming/).    With  the  use  of  the  parameterized  automatic
tool/blank  positioning  feature,  the  process  simulation  is  fully  automated  (no  user 
intervention required).  Based on the calculated spring back amount, tooling geometry 
is  compensated  through  a  compensation  run.    The  stamping  process  simulation  is 
conducted again, automatically, based on the new compensated tooling, followed by a 
second  tooling  compensation  (ITERATION  1).    Iterations  2,  3,  and  4  follow  the  same 
pattern.    The  iteration  process  is  repeated  until  blank  spring  back  shape  conforms  to 
tooling  designed  intent  (target),  or  until  it  reaches  4  iterations  (typically  required  to 
achieve part tolerance).  With some shell scripting this iterative loop can be completed 
automatically.  These tools allow the user to toggle between single and double precision 
version of LS-DYNA. 
The  task  of  tracking  the  files  involved  in  the  iterative  process  can  be  daunting, 
especially in the advanced stage of the iterations.  Figure 25-27 indicate what is written 
to storage during the process.
1_iter0.dir
sub-directories
1_gravity.dir
2_form.dir
sim_forming_mesh.k
3_trim.dir
dynain and geocur.trm
rigid.new
4_spbk.dir
dynain
5_comp.dir
geotrm.new
disp.tmp
geotrm.new
rigid.new
2_iter1.dir
sub-directories
1_gravity.dir
2_form.dir
3_trim.dir
dynain 
4_spbk.dir
dynain
5_comp.dir
disp.tmp
geotrm.new
rigid.new
5_iter4.dir
4_iter3.dir
rigid.new
3_iter2.dir
sub-directories
sub-directories
geotrm.new
sub-directories
1_gravity.dir
2_form.dir
3_trim.dir
4_spbk.dir
rigid.new
geotrm.new
1_gravity.dir
2_form.dir
3_trim.dir
dynain 
4_spbk.dir
dynain
5_comp.dir
1_gravity.dir
2_form.dir
3_trim.dir
dynain 
4_spbk.dir
dynain
5_comp.dir
disp.tmp
geotrm.new
rigid.new
Figure 25-27.  File structure for compensation 
An  input  deck  defining  a  spring  back  compensation  model  is  given  below.    The 
keyword file blank0.k includes node and element information of the blank shape before 
spring  back  (after  forming  and  trimming)  with  adaptive  constraints  (if  exist).    The 
keyword  file  spbk.k  includes  node  and  element  information  of  the  blank  after  spring 
back,  with  adaptive  constraints  (if  they  exist).    The  blank  shapes  before  and  after 
springback  (blank0.k  and  spbk.k)  may  be  based  on  either  the  original  die  design 
(ITER0), or based on an intermediate compensated die design (say the nth iteration). 
The  keyword  file  reference0.k  is  the  blank  shape  before  spring  back  for  iteration  0 
(ITER0).    This  file  is  blank0.k  and  should  not  change  from  iteration  to  iteration.    For 
iteration  0  the  file  reference1.k  is  also  the  same  as  blank0.k,  but  for  iteration  1 
refereince1.k  should  be  the  disp.tmp  generated  from  the  compensation  calculation 
during iteration 0 and so on and so forth for the subsequent iterations.
The  keyword  input  tools.k  must  contain  the  mesh  information  for  all  of  the  stamping 
tools in their home positions.  Compensated tools will be written to rigid.new with the 
original  constant  gap  being  maintained  among  the  tools.    During  the  baseline 
calculation, iteration 0, a keyword file called geocur.trm, generated during a LS-DYNA 
trimming  simulation  based  on  trimming  curve  input  (usually  in  IGES  format),  is  used 
for  keyword  *INCLUDE_COMPENSATION_TRIM_CURVE.    In  the  compensation  run 
of the ITER1, geocur.trm is used to generate new trim curves called geotrm.new, which 
conforms to the current compensated tools; and this new mapped trim curves are used 
for the ensuing ITER2, so on and so forth.  The new trim file, geotrm.new is also is also 
in keyword format and contains a *DEFINE_CURVE_TRIM_3D card. 
In  the  example  below  models  a  three-piece  air  draw  process.    The  upper  die  cavity 
(including binder) has a part ID 2, which is included in the part set ID 1 and is used for 
variable PSIDM.  Method 8 will compensate all the tools included in file tools.k based 
on compensated shape for the upper cavity. 
*KEYWORD 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- 
*INTERFACE_COMPENSATION_NEW 
$   METHOD        SL        SF     ELREF     PSIDm    UNDRCT    ANGLE NLINEAR 
         8    10.000     1.000         0         1         0      0.0       1 
*INCLUDE_COMPENSATION_BLANK_BEFORE_SPRING BACK 
blank0.k 
*INCLUDE_COMPENSATION_BLANK_AFTER_SPRINBACK 
spbk.k 
*INCLUDE_COMPENSATION_DESIRED_BLANK_SHAPE 
reference0.k 
*INCLUDE_COMPENSATION_COMPENSATED_SHAPE 
reference1.k 
*INCLUDE_COMPENSATION_CURRENT_TOOLS 
tools.k 
*INCLUDE_COMPENSATION_TRIM_CURVE 
geocur.trm 
*SET_PART_LIST 
$      PSID 
         1 
$      PID 
         2 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- 
*END 
NUMISHEET 2005: 
In  Figure  25-28,  the  NUMISHEET  2005  cross  member  is  compensated  following  the 
flow chart.  In two iterations the spring back is reduced from 13mm to 1.7mm.  Further 
iterations  will  reduce  the  part  deviation  down  to  a  specific  design  target.    Typically, 
four iterations are needed.
Iterative compensation applied during die construction 
The blank shape after spring back can be obtained from the actual experimental shape 
of  the  spring  back  panel,  if  available.    For  example,  in  hard  tool  construction,  the 
trimmed panel can be scanned using white light technology and the panel shape can be 
written to an STL file.  The STL format can  be easily converted to LS-DYNA keyword 
format  and  the  trimmed  panel  can  be  used  as  a  rigid  tool  onto  which  the  baseline 
(ITER0)  trimmed  panel  (deformable)  can  be  “pushed”  using  element  normal  pressure, 
and  using  *CONTROL_IMPLICIT_FORMING  type  1.    In  this  scenario,  the  adaptive 
refinement is turned off to maintain the one-to-one correspondence of the elements and 
nodes information.  An advantage of this method is that the spring back shape used for 
compensation will be exactly the same as the actual panel spring back, therefore the best 
tooling compensation result is expected.  An example of such is shown in Figures 25-29 
and 25-30. 
Compensation of localized regions 
Compensation of a localized tooling region is possible, with the keyword *INCLUDE_-
COMPENSATION_CURVE,  by  incorporating  the  following  lines  into  the  above 
example inputs: 
*INCLUDE_COMPENSATION_CURVE 
curves.k 
The file curves.k defines the two enclosed “begin” and “end” curves using *DEFINE_-
CURVE_COMPENSATION_CONSTRAINT_BEGIN/END.    More  explanations  can  be 
found  in  the  corresponding  keyword  manual  entries.    In  Figure  25-31,  the  NUMISH-
EET’05  decklid  inner  is  compensated  locally  in  the  horizontal  area  above  the  backlite.  
Tangency  of  the  compensated  tool  is  maintained  at  the  “End  Curve”  as  shown  in  the 
section  A-A.    Also  shown  in  Figure  25-32  includes  color  contours  of  part-separation 
distance  throughout  the  iterations  between  compensated  panel  and  the  target  design 
intent.  Part tolerance is achieved in two iterations. 
Accelerated spring back compensation (ASC) 
The option ACCELERATOR can be used in conjunction with *INCLUDE_COMPENSA-
TION,  with  options  ORIGINAL_DYNAIN  and  SPRING  BACK_INPUT  to  compensate 
spring back with a faster convergence rate and a simplified user interface.  A complete 
example is provided below.  The example uses a spring back input file spbk.dyn, and a 
trimmed  panel,  with  file  name  case20trimmed.dynain  (including  all  stress  and  strain 
tensors  and  adaptive  constraints).    The  variable  ISTEPS  is  increased  from  0  to  3, 
representing 3 compensation iterations.  ISTEPS = 0 represents the baseline spring back 
simulation (ITER0);  while ISTEPS = 1, 2, 3 represent the compensation iterations.  This 
feature  requires  the  user  to  change  only  one  variable  (ISTEPS),  and  then  submit  the 
same input file to continue the next iteration.
Many  scratch  files,  including  a  file  named  acceltmp.tmp,  will  be  generated.    Do  not 
delete  them.    They  are  used  to  pass  data  between  steps.    A  file,  compensation.info,  is 
generated and updated after each ISTEPS calculation.  It contains iteration information, 
including  maximum  deviations  in  the  𝑥,  𝑦,  and  𝑧  directions.    When  the  maximum 
deviation  is  within  the  tolerances  specified  in  the  TOLX,  TOLY,  and  TOLZ  fields,  a 
message  appears  in  the  file  indicating  the  compensation  iterations  have  converged, 
along with a message bootstrapping the next step.  A file spbk.new is generated in the 
same  directory  and  is  used  by  the  *INCLUDE_COMPENSATION_BLANK_AFTER_-
SPRING  BACK  keyword  with  the  scale  factor  for  the  tool  compensation  set  to  one.  
After the compensation, a verification calculation may be needed. 
*KEYWORD 
*INTERFACE_COMPENSATION_NEW_ACCELERATOR 
$   ISTEPS      TOLX      TOLY      TOLZ    OPTION 
         3      0.20      0.20       0.2         1 
*INCLUDE_COMPENSATION_ORIGINAL_DYNAIN 
./case20trimmed.dynain 
*INCLUDE_COMPENSATION_SPRING BACK_INPUT 
./spbk.dyn 
*END 
Currently,  mesh  coarsening  and  checking  are  not  supported  in  the  accelerated  mode.  
Also, the dynain file from the previous die process is not necessary. 
An example of this feature is shown for a simple channel type of draw (one-half model) 
in Figure 25-33, which converged in three iterations; while four iterations were needed 
for the non-accelerated compensation. 
Line die compensation 
The option MULTI_STEPS can be used together with *INCLUDE_COMPENSATION_-
COMPENSATED_SHAPE_NEXT_STEP to enable compensation of tools for the next die 
process.    An  example  is  given  below.    In  this  example  the  target  blank,  named 
reference0.tmp,  and  the  current  tool  named  rigid.tmp  come  from  the  first  die  process.  
The  disp.tmp  file  comes  from  the  compensation  in  the  second  die  process  step.    For 
example, a flanging die compensation can be a second die process step, preceded by a 
redraw die process as the first die process step. 
*KEYWORD 
*INTERFACE_COMPENSATION_NEW_MULTI_STEPS 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
$   METHOD        SL        SF     ELREF      PSID    UNDRCT     ANGLE   NLINEAR 
         8     6.000      1.00         1         1         0         0         1 
*INCLUDE_COMPENSATION_DESIRED_BLANK_SHAPE 
reference0.tmp 
*INCLUDE_COMPENSATION_COMPENSATED_SHAPE_NEXT_STEP 
disp.tmp 
*INCLUDE_COMPENSATION_CURRENT_TOOLS 
rigid.tmp 
*SET_PART_LIST
$      PSID 
          1 
$       PID 
          2 
*END 
Compensation of trim dies (trim die nesting) 
The  trim  die  can  be  compensated  using  the  drawn  panel’s  springnack  shape  when 
METHOD is set to -8.  In the example below, which is also shown in Figure 25-34, the 
draw panel, state1.k, is taken as the blank before spring back, and, draw panel spring 
back  shape,  state2.k,  is  taken  as  the  blank  after  spring  back.    The  tool  shape  for  the 
draw  process,  drawtool.k,  is  used  as  the  current  tool.    After  the  simulation,  LS-DYNA 
will  create  a  compensated  tool  named  rigid.new,  which  can  be  used  for  the  trim  die 
shape. 
*KEYWORD 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*INTERFACE_COMPENSATION_NEW 
$   METHOD        SL        SF     ELREF      PSID    UNDRCT     ANGLE   NLINEAR 
        -8    10.000     1.000         2         1         0       0.0         1 
*INCLUDE_COMPENSATION_BLANK_BEFORE_SPRINGBACK 
state1.k 
*INCLUDE_COMPENSATION_BLANK_AFTER_SPRINGBACK 
state2.k 
*INCLUDE_COMPENSATION_DESIRED_BLANK_SHAPE 
ref0.tmp 
*INCLUDE_COMPENSATION_COMPENSATED_SHAPE 
ref1.tmp 
*INCLUDE_COMPENSATION_CURRENT_TOOLS 
drawtool.k 
*INCLUDE_COMPENSATION_TRIM_CURVE 
orginaltrim.k 
*SET_PART_LIST 
$      PSID 
         1 
$      PID 
         3 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*END 
Local smoothing of tooling mesh: 
The  option  LOCAL_SMOOTH  can  be  used,  along  with  a  few  more  keywords,  to 
smooth  and  restore  the  distorted  tooling  mesh  after  iterative  compensation.    In  the 
example  below,  the  keyword  *INCLUDE_COMPENSATION_ORIGINAL_RIGID_-
TOOL  includes  an  original  tool,  rigid.tmp,  which  has  a  good  and  smooth  mesh.    The 
keyword  *INCLUDE_COMPENSATION_NEW_RIGID_TOOL  includes  a  compensated 
tool, rigidnew.bad, which could have a distorted mesh arising from the reasons listed in 
the “Purpose” section of this keyword. 
The last keyword *SET_NODE_LIST_SMOOTH defines a node set in and surrounding a 
distorted  local  area  in  the  distorted  mesh.    Each  node  set  defines  a  region  needing
smoothing.  The node set should not include any boundary nodes of the tooling parts, 
otherwise  position  of  the  tooling  may  be  altered  undesirably.    Smoothed  tooling  is 
stored in a file called rigid.new.  In this example method 7 is active, the variable ELREF 
is  set  to  2,  and  PSID  left  as  undefined.    Note  also  the  *INCLUDE  keyword  is  not 
supported here.  For example, *SET_NODE_LIST_SMOOTH must not be in a separate 
file and included in the main input file. 
*KEYWORD 
*INTERFACE_COMPENSATION_NEW_LOCAL_SMOOTH 
$   METHOD        SL        SF     ELREF      PSID    UNDRCT     ANGLE   NLINEAR 
         7    10.000     1.000         2                   0       0.0         1 
*INCLUDE_COMPENSATION_ORIGINAL_RIGID_TOOL 
rigid.tmp 
*INCLUDE_COMPENSATION_NEW_RIGID_TOOL 
rigidnew.bad 
*SET_NODE_LIST_SMOOTH 
         1  
     61057     61058     61059     61060     61061     61062     61063     61064 
... 
*SET_NODE_LIST_SMOOTH 
         2  
     56141     56142     56143     56144     56145     56146     56147     56148 
... 
*END 
In  an  example  shown  in  Figures  25-35  and  25-36,  smoothing  of  the  local  mesh  is 
performed in the draw bead area of the NUMISHEET 2005 cross member.  In this case 
the die gap is not maintained throughout the tooling surface.  Typically this happens in 
the draw bead regions when male beads have lower bending radii (missing upper radii) 
and female beads have only upper bending radii (missing lower radii).  Two node sets 
are  defined  for  local  areas  of  left  and  right  female  draw  beads  (Figure  25-37),  which 
needed smoothing.  It is important to include in the node sets some of the nodes on the 
relatively  flat  portion  of  the  binder  immediately  off  the  bend  radii.    Smoothed  results 
show  original  distorted  meshes  on  the  lower  beads  corner  areas  are  corrected  and  is 
satisfactory, Figure 25-38. 
In another example, a corner of a flanging die on a fender outer is being smoothed.  The 
mesh becomes distorted after a few compensation iterations, as shown in Figure 25-39.  
In  Figure  25-40,  the  result  of  local  smoothing  is  shown,  and  the  improvement  is 
remarkable. 
Compensation with symmetric boundary condition 
A keyword example is provided in the manual pages related to *INCLUDE_COMPEN-
SATION_{OPTION}.
Global compensation using the original tool mesh 
For some tooling meshes, the compensated die surfaces will be distorted.  The keyword 
option  *INCLUDE_COMPENSATION_ORIGINAL_TOOL  causes  the  compensation 
code  to  use  the  original  tooling  mesh  (starting  in  the  second  compensation)  to 
extrapolate  the  addendum  and  binder  in  the  compensated  tooling  surfaces.    This 
minimizes  the  accumulative  error,  compared  with  using  the  last  compensated  tooling 
mesh, and therefore is a preferred method. 
A complete keyword example is included below.  In it, part ID 3 (included in part set ID 
1)  is  being  compensated  after  ITERATION  #3  (ITER3),  using  method  #8,  with  a  scale 
factor of 0.5.  The dynain files from the trimmed ITER3 is taken as the “BEFORE” state 
  and  the  dynain  file  from  the  springback 
calculation is taken as the “AFTER” state.  The “DESIRED” blank shape is given by the 
dynain  is  from  the  trimmed  ITER0  output.    The  “COMPENSATED_SHAPE”  is  taken 
from the disp.tmp  file of the last  compensation run.  “CURRENT_TOOL” is also  from 
last  compensation  iteration.    The  “ORIGINAL_TOOL”,  is  taken  from  the  tool  mesh  in 
ITER0.  Updated trim curves geotrm.new are taken from the mapped trim lines of last 
compensation. 
It should be noted that, in an automatic compensation-loop calculation, as shown in the 
path of the input files, input files disp.tmp, rigid.new, and geotrm.new, taken from the 
default file names of the previous compensation, should not be in the same directory as 
the current compensation run, as these files will be overwritten. 
*KEYWORD 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*INTERFACE_COMPENSATION_NEW 
$   METHOD        SL        SF     ELREF      PSID    UNDRCT     ANGLE   NLINEAR 
         8    10.000     0.500         2         1         1       0.0         1 
*INCLUDE_COMPENSATION_BLANK_BEFORE_SPRINGBACK 
../7_iter3.dir/2_trim.dir/dynain 
*INCLUDE_COMPENSATION_BLANK_AFTER_SPRINGBACK 
../7_iter3.dir/3_spbk.dir/dynain 
*INCLUDE_COMPENSATION_DESIRED_BLANK_SHAPE 
../1_iter0.dir/2_trim.dir/dynain 
*INCLUDE_COMPENSATION_COMPENSATED_SHAPE 
../6_compensation.dir/disp.tmp 
*INCLUDE_COMPENSATION_CURRENT_TOOLS 
../6_compensation.dir/rigid.new 
*INCLUDE_COMPENSATION_ORIGINAL_TOOLS 
../1_iter0.dir/sim_forming_mesh.k 
*INCLUDE_COMPENSATION_TRIM_CURVE 
../6_compensation.dir/geotrm.new 
*SET_PART_LIST 
$      PSID 
         1 
$      PID 
         3 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 
*END
Updating compensated tool with small amount of part shape change 
Often times a part will have some small amount of shape change as a result of a product 
change.    If  the  amount  of  shape  change  does  not  significantly  alter  the  spring  back 
results, the compensated tools can be updated with the part mesh (inside the trim lines) 
or  formed  blank  shape  without  going  through  another  iterative  compensation  loop.  
This  is  accomplished  using  the  PART_CHANGE  option.    Within  the  specified  MAX-
GAP,  compensated  tool  shape  can  be  updated.    Changes  to  geometry  involving  sharp 
corners and transition with no fillet are not permissible.  A complete keyword example 
is  provided  below,  where  a  maximum  gap  of  5mm  is  specified  between  the  original 
shape and modified product shape.  The updated part file name is updatepart.tmp and 
output file for the new rigid tool is newrigid.k. 
*KEYWORD 
*INTERFACE_COMPENSATION_NEW_PART_CHANGE 
$   MAXGAP 
       5.0 
*INCLUDE_COMPENSATION_DESIRED_BLANK_SHAPE 
../1_iter0.dir/2_trim.dir/dynain 
*INCLUDE_COMPENSATION_COMPENSATED_SHAPE 
../6_compensation.dir/disp.tmp 
*INCLUDE_COMPENSATION_CURRENT_TOOLS 
../6_compensation.dir/rigid.new 
*INCLUDE_COMPENSATION_UPDATED_BLANK_SHAPE 
./updatedpart.tmp 
*INCLUDE_COMPENSATION_UPDATED_RIGID_TOOL 
$ file name to output the new rigid tools 
./newrigid.k 
*END 
Option REFINE_RIGID: rigid tool mesh refinement for a better convergence 
The  following  keyword  example  refines  and  breaks  the  elements  in  the  original  tool 
mesh  file  rigid.new  along  provided  trim  curves  trimcurve106.k,  defined  using  the 
keyword  *DEFINE_CURVE_TRIM_3D.    The  refined  rigid  tool  mesh  will  be  output  as 
rigid_refined.tmp,  which  can  be  used  to  start  the  iterative  springback  compensation 
process. 
*KEYWORD 
*INTERFACE_COMPENSATION_NEW_REFINE_RIGID 
rigid.new 
trimcurve106.k 
*END 
Reference: 
The  manual  pages  related  to  *INCLUDE_COMPENSATION_{OPTION}  can  be  further 
referenced for details.
Revision Information: 
This keyword requires double precision executable.  The option of ACCELERATOR is 
available starting in Revision 61264.  The option of MULTI_STEPS is available starting 
in  Revision  61406.    The  option  of  LOCAL_SMOOTH  is  available  starting  in  Revision 
73850.    The  keyword  option  *INCLUDE_COMPENSATION_ORIGINAL_TOOL  is 
available starting in Revision 82701.  The keyword option PART_CHANGE is available 
starting in Revision 82698.  The REFINE_RIGID option is available starting in Revision 
113089.
Nominal 
Surface
■ ITERATION 0
■ Max. springback 13mm on flanges
Trim Panel 
Springback
■ ITERATION 1
■ Springback reduced to < 3.5mm
Springback Covergence (mm)
15.0
10.0
5.0
0.0
■ ITERATION 2
■ Springback reduced to < 1.7mm
Max Deviation 
1.7m 
ITER0  ITER1   ITER2
■ Compensation convergence history
Symmetry 
Plane
Upper Die Cavity
Sheet Blank
Trim Lines
Lower Binder
Lower Post
Drawn Panel
2005 NUMISHEET Cross Member Model
Drawn Panel and Trim Lines
Figure  25-28. 
Xmbr(red – springback, blue – design intent) 
  Iterative  springback  compensation  on  NUMISHEET’05
Scan data from (STL) 
"Pushed in"  blank
Figure 25-29.  A trimmed panel “pushed” onto the scan data (rigid body). 
Figure 25-30.  Section showing the “push” results – before and after.
Begin curve
Transition region
End curve
Figure 25-31.  Two curves defining a localized area of a decklid inner. 
Section A-A
ITER0
ITER1
ITER2
Distance to 
target (mm)
3.5
3.0
2.5
2.0
1.5
1.0
0.5
0.0
Figure 25-32.  Iterative compensation for a localized (backlite) region.
Distance to target (mm) with
 ISTEP=0~3, 1 verification run
0.5
0.4
0.3
0.2
0.1
0.0
ITER0 trim panel
ITER0 springback
Original tools
Accelerated Springback Compensation 
Figure 25-33.  Accelerated Springback Compensation. 
rigid.new
(compensated draw tools 
for trim die)
drawtool.k
state1.k
(drawn panel)
state2.k
(drawn panel springback)
Figure 25-34.  Trim die compensation with drawn panel springback shape.
Figure 25-35.  The NUMISHEET 2005 cross member. 
Figure 25-36.  Multiple sections cut on the lower binder.
Node set 1
Node set 2
Figure 25-37.  Local smoothing - two node sets defined including some nodes 
on the relatively flat binder area for both left and right draw beads. 
Original distorted
Smoothed
  Figure 25-38.  Comparison between original and smoothed tooling mesh.
Figure 25-39.  Original distorted tooling mesh. 
Figure 25-40.  Smoothed tooling mesh.
*INTERFACE_COMPONENT_FILE 
Purpose:    Allow  for  the  specification  of  the  file  where  the  component  interface  data 
should be written, and the optional use of a new binary format for that data. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
Optional Card. 
Filename 
A80 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Format 
Type 
Default 
I 
2 
  VARIABLE   
DESCRIPTION
FNAME 
Name of the file where the component data will be written 
FORMAT 
File format to use: 
EQ.1: Use old binary file format 
EQ.2: Use new LSDA file format 
Remarks: 
If Z = is used on the command line, this card will be ignored.  If this card is in effect, the 
new  LSDA  file  format  is  the  default  format  to  be  used.    The  new  format  has  certain 
advantages, and one possible drawback: 
1. 
It allows for the use of the_TITLE modifier on all *INTERFACE_COMPONENT 
inputs,  so  that  subsequent  *INTERFACE_LINKING  cards  can  refer  to  compo-
nents by a user specified ID.
2. 
3. 
It is fully portable between machines with different precision and byte order. 
It maintains the full precision of the coordinate vector.  The internal coordinate 
vector has been in double precision for quite some time, even for single preci-
sion executables.  The  old binary format writes 32 bit data for single precision 
executables, losing some precision in the process. 
4.  Because  of  the  maintained  precision,  the  new  format  files  will  be  significantly 
larger when running in single precision. 
Of  course,  the  new  file  format  cannot  be  used  for  subsequent  analysis  with  older 
versions of LS-DYNA, particularly those with a Product ID less than 50845.  Executables 
which can read the new format for *INTERFACE_LINKING analysis will automatically 
detect whether the new or old format is in use.
*INTERFACE_COMPONENT_OPTION1_{OPTION2} 
Available values for OPTION1 include: 
NODE 
SEGMENT 
OPTION2 only allows the value: 
TITLE 
Purpose:  Create an interface for use in subsequent linking calculations.  This command 
applies to the first analysis for storing interfaces in the interface file specified either by 
“Z=isf1” on the execution line or by the *INTERFACE_COMPONENT_FILE command.  
The  output  interval  used  to  write  data  to  the  interface  file  is  controlled  by  OPIFS  on 
*CONTROL_OUTPUT.    If  OPIFS  is  not  specified,  the  interval  defaults  to  1/10th  the 
value of DT specified in *DATABASE_BINARY_D3PLOT. 
This  capability  allows  the  definition  of  interfaces  that  isolate  critical  components.    A 
database  is  created  that  records  the  motion  of  the  interfaces.    In  later  calculations  the 
isolated components can be reanalyzed with arbitrarily refined meshes with the motion 
of  their  boundaries  specified  by  the  database  created  by  this  input.    The  interfaces 
defined here become the masters in the tied interface options. 
Each  definition  consists  of  a  set  of  cards  that  define  the  interface.    Interfaces  may 
consists of a set of segments for later use with *INTERFACE_LINKING_SEGMENT, an 
ordered line of nodes for use with *INTERFACE_LINKING_EDGE, or an unordered set 
of nodes for use with *INTERFACE_LINKING_NODE.   
Title Card.  Additional card for TITLE keyword option. 
  Card 1 
Variable 
1 
ID 
Type 
I 
Default 
none 
2 
3 
4 
5 
6 
7 
8 
Title 
A70 
None 
  VARIABLE   
DESCRIPTION
ID 
Title 
LS-DYNA R10.0 
ID for this interface in the linking file
Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
CID 
NID 
Type 
I 
I 
I 
  VARIABLE   
DESCRIPTION
Set ID, see *SET_NODE or *SET_SEGMENT. 
Coordinate system ID 
Node ID 
SID 
CID 
NID 
Remarks: 
CID  and  NID  are  optional.    If  CID  appears,  the  transformation  matrix  for  this 
coordinate system is written to the linking file at each output state.  If NID appears, the 
displacement of this node is also written to the file.  This information is then available to 
be  used  by  the  *INTEFACE_LINKING_NODE_LOCAL.    If  either  of  these  is  non-zero, 
then  the  linking  file  will  be  written  in  the  LSDA  format,  as  the  old  format  cannot 
support this optional output. 
If  the  old  style  binary  format  is  used  for  the  linking  file    then  the  ID  values  are  ignored  and  all  components  are  numbered 
according to their input order, starting from 1.
*INTERFACE 
Purpose:    Define  the  failure  models  for  bonds  linking  various  discrete  element  (DE) 
parts within one heterogeneous bond (*DEFINE_DE_HBOND). 
2 
3 
4 
5 
6 
7 
8 
  Card 1 
Variable 
1 
IID 
Type 
I 
Default 
none 
Bond  Definition  Cards.    For  each  bond  definition,  include  an  additional  card.    This 
input ends at the next keyword (“*”) card.  
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID1 
PID2 
PTYPE1 
PTYPE2 
FRMDL 
FRGK 
FRGS 
DMG 
Type 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
I 
1 
F 
F 
F 
none 
none 
1.0 
  VARIABLE   
DESCRIPTION 
IID 
PID1 
Interface ID.  All interfaces should have a unique ID 
First part ID.
VARIABLE   
PID2 
DESCRIPTION 
Second  part  ID.    PID1  and  PID2  define  the  bonds  that  this  fracture
model is applied to.  There are three combinations as 
Case a:  PID1.EQ.0 
This  is  the  default  model  for  all  bonds,  overriding  the  de-
fault model defined in Card 2 of *DEFINE_DE_HBOND. 
Case b:  PID1.GT.0 and PID2.EQ.0 
This model is applied to the bonds within part PID1, instead
of the default model. 
Case c:  PID1.GT.0 and PID2.GT.0 
This model is applied to the bonds between parts PID1 and
PID2 only, but not to those within part PID1 or part PID2 (as 
in case b). 
Notes: 
1.  The default fracture model is applied to all parts that are not
specified in case b. 
2.  The  fracture  model  of  the  part  with  a  smaller  part  id  is
applied to the bonds between two different parts if not spec-
ified in case c. 
PTYPE1 
First part type: 
EQ.0:  DES part set 
EQ.1: DES part 
PTYPE2 
Second part type: 
EQ.0:  DES part set 
EQ.1: DES part 
FRMDL 
Fracture model.  (same as FRMDL in Card2 of keyword *DEFINE_-
DE_HBOND.) 
FRGK 
FRGS 
DMG 
Fracture  energy  release  rate  for  volumetric  deformation.    (same  as
FRGK in Card2 of keyword *DEFINE_DE_HBOND.) 
Fracture  energy  release  rate  for  shear  deformation.    (same  as  FRGS
in Card 2 of keyword *DEFINE_DE_HBOND.) 
Continuous  damage  development.    (same  as  DMG  in  Card  2  of
keyword *DEFINE_DE_HBOND.)
INTERFACE_DE_HBOND EXAMPLE: 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  *INTERFACE_DE_HBOND 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$  Using DE_HBOND to bond 4 parts with different failure models 
$ 
*SET_PART_LIST_TITLE 
DES BOND PARTS 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      sid       da1       da2       da3       da4  
         1 
$      id1       id2       id3       id4 
       101       102       103       104 
*SET_PART_LIST_TITLE 
DES HBOND SUB PARTS 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      sid       da1       da2       da3       da4  
         2 
$      id1       id2 
       103       104 
*INTERFACE_DE_HBOND 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      iid 
         1 
$     pid1      pid2    ptype1    ptype2     frmdl      frgk      frgs       dmg  
       101         0         1         0         1     1.0E1     1.0E1       1.0 
         2         0         0         0         1     1.0E3     1.0E3       1.0 
       102       103         1         1         2     1.0E2     1.0E2       1.0 
$ 
*DEFINE_DE_HBOND 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      sid     stype    bdform      idim 
         1         2         2         3 
$   pbk_sf    pbs_sf      frgk      frgs     bondr     alpha       dmg     frmdl 
         1         1     1.0E0     1.0E0       2.5      0.01       1.0         1 
$   precrk    cktype               itfid 
         0         0                   1 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ the fracture models for the bonds within each part are determined as 
$ 
$   pid1    pid2    frgk    comments 
$    101     101   1.0E1    Line 1 in the interface card 
$    102     102   1.0E0    default (defined in hbond card) 
$    103     103   1.0E3    Line 2 in the interface card 
$    104     104   1.0E3    Line 2 in the interface card 
$ 
$ for the bonds between two parts: 
$    101     102   1.0E1    taken from Part 101 (smaller part id) 
$    101     103   1.0E1    taken from Part 101 (smaller part id) 
$    101     104   1.0E1    taken from Part 101 (smaller part id) 
$    102     103   1.0E2    Line 3 in the interface card 
$    102     104   1.0E0    taken from Part 102 (smaller part id) 
$    103     104   1.0E3    taken from Part 103 (smaller part id) 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
*INTERFACE_LINKING_DISCRETE_NODE_OPTION 
Available options include: 
NODE 
SET 
Purpose:  Link node(s) to an interface in an existing interface file.  This link applies to all 
element types.  The interface file is specified using *INTERFACE_LINKING_FILE or by 
including “L=filename” on the execution line.   
With this command, nodes in a node set must be given in the same order as they appear 
in the interface file.  This restriction does not apply to the more recent keyword *INTER-
FACE_LINKING_NODE_…. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  NID/NSID 
IFID 
Type 
I 
I 
  VARIABLE   
NID 
DESCRIPTION
Node ID or Node set ID to be moved by interface file, see *NODE
or *SET_NODE. 
IFID 
Interface ID in interface file.
*INTERFACE 
Purpose:    Link  a  series  of  nodes  to  an  interface  in  an  existing  interface  force  file.    The 
including 
interface  file 
“L=filename” on the execution line. 
is  specified  using  *INTERFACE_LINKING_FILE  or  by 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSID 
IFID 
Type 
I 
I 
  VARIABLE   
DESCRIPTION
Node set ID to be moved by interface file. 
Interface ID in interface file. 
NSID 
IFID 
Remarks: 
The  set  of  nodes  defined  will  be  constrained  to  follow  the  movement  of  the  interface 
IFID,  which  should  correspond  to  a  curve  output  on  a  previous  analysis  via  *INTER-
FACE_COMPONENT_NODE.  The order of the nodes in the first analysis is important.  
The nodes, in the order specified in the first analysis, represent a curve.  Each node in 
set  NSID  will  be  tied  to  the  point  on  the  curve  nearest  to  its  initial  position,  and  then 
will  be  constrained  to  follow  that  point  on  the  curve  for  the  duration  of  the  analysis.  
This  option  is  intended  to  be  used  with  beam  or  shell  elements,  as  both  translational 
and rotational degrees of freedom are constrained.
*INTERFACE_LINKING_FILE 
Purpose:    Allow  for  the  specification  of  the  file  from  which  the  component  interface 
data should be read. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
Filename 
A80 
none 
  VARIABLE   
DESCRIPTION
FNAME 
Name of the file from which the component data will be read 
Remarks: 
If  L=  is  used  on  the  command  line,  this  card  will  be  ignored.    There  is  no  option  to 
specify the file format, as the file format is automatically detected.
*INTERFACE_LINKING_NODE_OPTION 
Available options include: 
SET 
LOCAL 
SET_LOCAL 
Purpose:  Link nodes(s) to an interface in an existing interface file.  This link applies to 
all element types.  The interface file is specified using *INTERFACE_LINKING_FILE or 
by including “L=filename” on the execution line. 
Node/Set ID Card.  Include as many cards as desired.  Input ends at the next keyword 
(“*”) card. 
  Card 1 
1 
2 
Variable  NID/NSID 
IFID 
Type 
I 
I 
3 
FX 
I 
4 
FY 
I 
5 
FZ 
I 
  VARIABLE   
DESCRIPTION
6 
7 
8 
NID 
IFID 
FX 
FY 
FZ 
Node ID or Node set ID to be moved by interface file, see *NODE 
or *SET_NODE. 
Interface ID in interface file. 
The  ID  of  a  *DEFINE_FUNCTION  which  determines  the  𝑥
direction displacement scale factor 
The  ID  of  a  *DEFINE_FUNCTION  which  determines  the  𝑦
direction displacement scale factor 
The  ID  of  a  *DEFINE_FUNCTION  which  determines  the  𝑧
direction displacement scale factor
Card 2.  This card appears after Card 1 when the_LOCAL option is used 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
LNID 
USEC 
USEN 
Type 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
Local coordinate system ID for transforming displacements. 
Local node ID for transforming displacements 
0/1 flag to indicate the use of the coordinate system in the linking
file during displacement transformation 
0/1  flag  to  indicate  the  use  of  the  node  displacement  in  the
linking file during displacement transformation. 
LCID 
LNID 
USEC 
USEN 
Remarks: 
The  set  of  nodes  is  constrained  to  follow  the  displacement  of  the  interface  having  ID 
IFID in the linking file.  Note that the linking file is usually generated by the *INTER-
FACE_COMPONENT_NODE kekyword in a previous analysis. 
The order of the nodes is not important.  Each node in set NID will be tied to the nearest 
node in IFID using a bucket sort during the initialization phase.  Nodes not found are 
reported  and  subsequently  not  constrained.    Translational  degrees  of  freedom  are 
constrained.    If  the  constrained  analysis  has  rotational  degrees  of  freedom,  then  the 
rotation  degrees  of  freedom  will  be  likewise  constrained  and  the  linking  file  must 
include rotational degrees of freedom. 
The displacements in the linking file can be scaled upon input so that 
𝐮constrained
=
𝑓FX(… )
⎡
⎢
⎣
𝑓FY(… )
⎤
⎥
𝑓FZ(… )⎦
𝐮linking file 
where 𝑓FX(… ) is the *DEFINE_FUNCTION function having ID FX and so on.  When a 
scaling function is not specified the corresponding component is imported unscaled as 
if the scaling function had a constant value of unity.  These functions may take either 0, 
1, 3, or 4 input arguments.  The functions FX, FY, and FZ may be different and they may 
take  different  numbers  of  arguments.    The  data  passed  into  the  scaling  function
depends on the number of arguments that the function takes and the possibilities can be 
broken down into four cases: 
1. 
2. 
3. 
4. 
0  variables.    A  function  taking  no  inputs  is  evaluate  constant  over  space  and 
time.    LS-DYNA  evaluates  such  a  function  at  the  start  of  the  calculation  and 
uses that value for the duration of the run. 
1  varriables.    LS-DYNA  passes  in  the  simulation  time  at  each  step  and  the 
resulting value is applied to all nodes in the set. 
3 varriables.  LS-DYNA passes in the initial position of each constrained node as 
an  (𝑥, 𝑦, 𝑧)  triple  at  the  start  of  the  calculation  and  then  uses  the  result  for  the 
duration of the run. 
4  varriables.    LS-DYNA  passes  in  the  current  simulation  time  and  the  initial 
position of each of the constrained nodes as an (𝑥, 𝑦, 𝑧, 𝑡) tuple.  This function is 
updated at each time step.  Using scaling functions of 4 variables may result in 
a performance penalty as each function must be evaluated for every slave node 
every cycle. 
If  time  dependent  scaling  functions  are  used,  then  the  constrained  nodes  must  start 
with coordinates identical to the constraining nodes in the linking file. 
The LOCAL option and the values of the LCID, LNID, USEC, USEN flags, which  was 
designed  in  conjunction  with  Honda  R&D  Co.,  Ltd.,  allow  for  the  interface 
displacements to be transformed in various ways.  By default, the scale factors FX, FY, 
FZ  act  on  the  nodal  displacements  in  the  global  coordinate  system  of  the  constrained 
calculation.  This may be undesirable depending on how the global coordinate system 
of the linked calculation is defined.  The most general transformation rule is: 
𝐮constrained = 𝐐2
𝑓FX(… )
⎡
⎢
⎣
𝑓FY(… )
⎤
⎥
𝑓FZ(… )⎦
𝐐𝟏(𝐮linked − 𝐜𝟏) − 𝐜𝟐 
where, 
𝐜1 = The displacement of the NID node in the linking file 
𝐜𝟐 = The displacement of node LNID 
𝐐1 = Rotation into the local coordinates of the linking file 
𝐐2 = Rotation into the local coordinate system, if unset the inverse of 𝐐1 
If  USEC = 0, then 𝐐1 is the identity rotation and any coordinate system in the linking 
file is ignored.  If USEN = 0, then 𝐜1 is set to 0 and NID in the linking file is ignored.
*INTERFACE_LINKING_SEGMENT 
Purpose:  Link segments to an interface in an existing interface file.  The interface file is 
specified  using  *INTERFACE_LINKING_FILE  or  by  including  “L=filename”  on  the 
execution line. 
Segment  Set  ID  Card.    Include  as  many  cards  as  desired.    Input  ends  at  the  next 
keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
IFID 
Type 
I 
I 
  VARIABLE   
DESCRIPTION
Segment set to be moved by interface file. 
Interface ID in interface file. 
SSID 
IFID 
Remarks: 
The set of segments defined will be constrained to follow the movement of the interface 
IFID, which should correspond to an interface output on a previous analysis using the 
*INTERFACE_COMPONENT_SEGMENT keyword.  The behavior will be the same as if 
set  SSID  is  the  slave  side  of  a  *CONTACT_TIED_SURFACE_TO_SURFACE  with  IFID 
as the master.  Translational movement will be constrained, but not rotations.
*INTERFACE_SPRINGBACK_OPTION1_OPTION2 
Available options included for OPTION1 are: 
LSDYNA 
NASTRAN 
SEAMLESS 
EXCLUDE  
and for OPTION2: 
THICKNESS 
NOTHICKNESS 
See Remark 1. 
Purpose:    Define  a  material  subset  for  an  implicit  springback  calculation  in  LS-DYNA 
and any nodal constraints to eliminate rigid body degrees-of-freedom. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PSID 
NSHV 
FTYPE 
FTENSR  NTHHSV 
INTSTRN 
Type 
I 
I 
I 
I 
I 
I 
Irregular Optional Card.  The keyword reader will interpret the card following Card 1 
as  new  optional  Card  2  if  the  first  column  of  the  card  is  occupied  by  the  string 
“OPTCARD”.  Otherwise, it is interpreted as first Node Card, see below. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OPTC 
SLDO 
NCYC 
FSPLIT 
NDFLAG 
Type 
A 
I 
I 
I
Node Cards.  Define a list of nodal points that are constrained for the springback.  This 
section is terminated by an “*” indicating the next input section. 
Card 
1 
Variable 
NID 
Type 
I 
2 
TC 
F 
3 
RC 
F 
4 
5 
6 
7 
8 
  VARIABLE   
DESCRIPTION
PSID 
NSHV 
Part set ID for springback, see *SET_PART. 
Number of shell or solid history variables (beyond the six stresses
and effective plastic strain) to be initialized in the interface file. 
For  solids,  one  additional  state  variable  (initial  volume)  is  also
written.    If  NSHV  is  nonzero,  the  element  formulations,  unit
system, and constitutive models should not change between runs.
If  NHSV  exceeds  the  number  of  integration  point  history
variables  required  by  the  constitutive  model,  only  the  number
required  is  written;  therefore,  if  in  doubt,  set  NHSV  to  a  large
number. 
FTYPE 
File type:  
EQ.0:  ASCII, 
EQ.1:  binary 
EQ.2:  both ASCII and binary. 
EQ.3:  LSDA format (for LSDYNA only) 
EQ.10:  ASCII large format  
EQ.11:  binary large format 
EQ.12:  both ASCII and binary large format 
FTENSR 
Flag for dumping tensor data from the element history variables
into the dynain file. 
EQ.0: Don’t dump tensor data from element history variables 
EQ.1: Dump  any  tensor  data  from  element  history  variables
into the dynain file in GLOBAL coordinate system.  Cur-
rently, only Material 190 supports this option.
VARIABLE   
DESCRIPTION
NTHHSV 
Number of thermal history variables. 
INTSTRN 
Output  of  strains  at  all  integration  points  of  shell  element  is
requested, see also *INITIAL_STRAIN_SHELL. 
SLDO 
Output of solid element data as 
EQ.0: *ELEMENT_SOLID, or 
EQ.1: *ELEMENT_SOLID_ORTHO. 
NCYC 
Number  of  process  cycles  this  simulation  corresponds  to  in  the 
simulation of wear processes, see Remark 6. 
FSPLIT 
Flag for splitting of the dynain file (only for ASCII format). 
EQ.0: dynain file written in one piece. 
EQ.1: Output  is  divided  into  two  files,  dynain_geo  including 
the geometry data and dynain_ini including initial stress-
es and strains. 
NDFLAG 
Flag to dump nodes into dynain file. 
EQ.0: default, dump only sph and element nodes 
NID 
TC 
EQ.1: dump all nodes 
Node ID, see *NODE. 
Translational Constraint: 
EQ.0: no constraints, 
EQ.1: constrained 𝑥 displacement, 
EQ.2: constrained 𝑦 displacement, 
EQ.3: constrained 𝑧 displacement, 
EQ.4: constrained 𝑥 and 𝑦 displacements, 
EQ.5: constrained 𝑦 and 𝑧 displacements, 
EQ.6: constrained 𝑧 and 𝑥 displacements. 
EQ.7: constrained 𝑥, 𝑦, and 𝑧 displacements.
VARIABLE   
DESCRIPTION
RC 
Rotational constraint: 
EQ.0: no constraints, 
EQ.1: constrained 𝑥 rotation, 
EQ.2: constrained 𝑦 rotation, 
EQ.3: constrained 𝑧 rotation, 
EQ.4: constrained 𝑥 and 𝑦 rotations, 
EQ.5: constrained 𝑦 and 𝑧 rotations, 
EQ.6: constrained 𝑧 and 𝑥 rotations, 
EQ.7: constrained 𝑥, 𝑦, and 𝑧 rotations. 
Remarks: 
1.  NOTHICKNESS  Option.    The  NOTHICKNESS  option  is  available  when  the 
keyword’s first option is either LS-DYNA or NASTRAN.  With the NOTHICK-
NESS option the shell element thickness is not output. 
2.  Filenames.    The  file  name  for  the  LS-DYNA  option  is  dynain  and  for  NAS-
TRAN is nastin. 
3.  Trimming.  Trimming is available for the adaptive mesh, but it requires manual 
intervention.  To trim an adaptive mesh use the following procedure: 
a)  Generate  the  file,  dynain,  using  the  keyword  *INTERFACE_SPRING-
BACK_LSDYNA. 
b)  Prepare a new input deck including the dynein file. 
c)  Add the keyword *ELEMENT_TRIM to this new deck. 
d)  Add the keyword *DEFINE_CURVE_TRIM to this new deck. 
e)  Run  this  new  input  deck  with  i=input_file_name.    The  adaptive  con-
straints are eliminated by remeshing and the trimming is performed. 
f) 
In case this new trimmed mesh is needed, run a zero termination time job 
and  output  the  file  generated  via  the  keyword,  *INTERFACE_SPRING-
BACK_LSDYNA. 
4.  Temperature.  The file new_temp_ic.inc will be created for a thermal solution 
and  a  coupled  thermal-mechanical  solution.    The  file  new_temp_ic.inc  is  a
KEYWORD  include  file  containing  new  temperature  initial  conditions  for  the 
nodes belonging to the PSID. 
a)  For  thermal  user  materials  it  is  possible  to  dump  thermal  history  varia-
bles.  See the NTHHSV field. 
5.  FTYPE.    The  choice  of  format  size  in  option  FTYPE  is  only  available  for  shell 
stresses  and  shell  history  data,  see  parameter  LARGE  on  *INITIAL_STRESS_-
SHELL.    For  solid  and  beam  elements,  always  the  large  format  is  written  to 
dynain, i.e.  LARGE is automatically set to 1 on *INITIAL_STRESS_SOLID and 
*INITIAL_STRESS_BEAM respectively. 
6.  NCYC. When simulating wear processes, this represents the number of process 
cycles  this  particular  simulation  corresponds  to  and  *INITIAL_CONTACT_-
WEAR  cards  are  generated  accordingly  in  the  dynain  file  (only  ascii  format 
supported).  Cards will only be generated for nodes in contact interfaces associ-
ated with a *CONTACT_ADD_WEAR, and having SPR or MPR set to 2 on the 
first  card  on  *CONTACT.    This  wear  data  is  in  a  subsequent  simulation  ac-
counted for NCYC times when modifying the worn geometry, or alternatively 
processed in LS-PrePost 
7.  EXCLUDE.    This  option  is  used  to  limit  what  data  will  be  output  to  the 
LSDYNA dynain file.  The input format is completely different, and consists of 
any number of keyword cards WITHOUT the leading *.  These cards and their 
associated data will not be output.  For example: 
*INTERFACE_SPRINGBACK_EXCLUDE 
BOUNDARY_SPC_NODE 
CONSTRAINED_ADAPTIVITY 
would output all the normal dynain data except for the SPC and adaptive con-
straints.  The currently recognized keywords that can be excluded are: 
BOUNDARY_SLIDING_PLANE 
BOUNDARY_SPC_NODE 
CONSTRAINED_ADAPTIVITY 
DEFINE_COORDINATE_NODES 
DEFINE_COORDINATE_VECTOR 
ELEMENT_BEAM 
ELEMENT_SHELL 
ELEMENT_SOLID 
INITIAL_STRAIN_SHELL 
INITIAL_STRAIN_SOLID 
INITIAL_STRESS_BEAM 
INITIAL_STRESS_SHELL
INITIAL_STRESS_SOLID 
INITIAL_TEMPERATURE_NODE 
INITIAL_VELOCITY_NODE 
NODE 
REFERENCE_GEOMETRY 
Remarks for Seamless Springback: 
When  seamless  springback  is  invoked,  the  solution  automatically  and  seamlessly 
switches  from  explicit  or  implicit  dynamic  to  implicit  static  mode  at  the  termination 
time, and continues to run the static  springback analysis.  Seamless springback  can  be 
activated in the original LS-DYNA input deck, or later using a small restart input deck.  
In this way, the user can decide to continue a previous analysis by restarting to add the 
implicit springback phase.  (Another alternative approach to springback simulation is to 
use the keyword *INTERFACE_SPRINGBACK_LSDYNA to generate a dynain file after 
forming,  and  then  perform  a  second  simulation  running  LS-DYNA  in  fully  implicit 
mode  for  springback.    See  Appendix  P  for  a  description  of  how  to  run  an  implicit 
analysis using LS-DYNA. 
The  implicit  springback  phase  begins  when  the  forming  simulation  termination  time 
ENDTIM  is  reached,  as  specified  with  the  keyword  *CONTROL_TERMINATION.  
Since  the  springback  phase  is  static,  its  termination  time  can  be  chosen  arbitrarily 
(unless material rate effects are included).  The default choice is 2.0 × ENDTIM, and can 
be  changed  using  the  *CONTROL_IMPLICIT_GENERAL  keyword;  see  variables  DT0 
and NSBS.. 
Since  the  springback  analysis  is  a  static  simulation,  a  minimum  number  of  essential 
boundary  conditions  or  Single  Point  Constraints  (SPC's)  can  be  input  to  prohibit  rigid 
body motion of the part.  These boundary conditions can be added for the springback 
input  option  on  the  *INTERFACE_SPRINGBACK_SEAMLESS 
phase  using  the 
keyword above. 
If  no  boundary  conditions  are  added  with  the  SEAMLESS  option  an  eigenvalue 
computation  is  automatically  performed  using  the  Inertia  Relief  Option  to  find  any 
rigid  body  modes  and  then  automatically  constrain  them  out  of  the  springback 
simulation  .    This  approach  introduces 
no artificial deformation and is recommended for many simulations. 
An  “SPR”  option  is  available  for  several  *CONTROL_IMPLICIT  keywords  to  further 
control the implicit springback phase.  Generally, default settings can be used, in which 
case the SPR option for *CONTROL_IMPLICIT keywords is not necessary. 
To  obtain  accurate  springback  solutions,  a  nonlinear  springback  analysis  must  be 
performed.    In  many  simulations,  this  iterative  equilibrium  search  will  converge
without  difficulty.    If  the  springback  simulation  is  particularly  difficult,  either  due  to 
nonlinear  deformation,  nonlinear  material  response,  or  numerical  precision  errors,  a 
multi-step  springback  simulation  will be automatically invoked.  In this approach, the 
springback deformation is divided into several smaller, more manageable steps. 
Two  specialized  features  in  LS-DYNA  are  used  to  perform  multi-step  springback 
analyses.    The  addition  and  gradual  removal  of  artificial  springs  is  performed  by  the 
artificial  stabilization  feature.   Simultaneously,  the  automatic  time step  control  is  used 
to guide the solution to the termination time as quickly as possible, and to persistently 
retry  steps  where  the equilibrium  search  has  failed.    By  default,  both  of  these  features 
are  active  during  a  seamless  springback  simulation.    However,  the  default  method 
attempts  to  solve  the  springback  problem  in  a  single  step.    If  this  is  successful,  the 
solution  will  terminate  normally.    If  the  single  step  springback  analysis  fails  to 
converge,  the  step  size  will  be  reduced,  and  artificial  stabilization  will  become  active.  
Defaults for these features can be changed using the following keywords: 
•  *CONTROL_IMPLICIT_GENERAL, 
•  *CONTROL_IMPLICIT_AUTO, and 
•  *CONTROL_IMPLICIT_STABILIZATION.
*INTERFACE_SSI 
Purpose:    This  card  creates  a  tied-contact  soil-structure  interface  for  use  in  a  transient 
analysis of a soil-structure system subjected to earthquake excitation.  This card allows 
the  analysis  to  start  from  a  static  state  of  the  structure,  as  well  as  to  read  in  ground 
motions recorded on the interface in an earlier analysis. 
Available options are: 
<BLANK> 
OFFSET 
CONSTRAINED_OFFSET 
LS-DYNA implements the effective seismic input method [Bielak and Christiano (1984)] 
for  modeling  the  interaction  of  a  non-linear  structure  with  a  linear  soil  foundation 
subjected to earthquake excitation.  Note that any non-linear portion of the soil near the 
structure may be incorporated with the structure into a larger generalized structure, but 
the soil is assumed to behave linearly beyond a certain distance from the structure. 
The  effective  seismic  input  method  couples  the  dynamic  scattered  motion  in  the  soil, 
which is the difference between the motion in the presence of the structure and the free-
field  motion  in  its  absence,  with  the  total  motion  of  the  structure.    This  replaces  the 
distant earthquake source with equivalent effective forces adjacent to the soil-structure 
interface and allows truncation of the large soil domain using a non-reflecting boundary 
(e.g.  *MAT_PML_ELASTIC) to avoid unnecessary computation.  These effective forces 
can be computed using the free-field ground motion at the soil-structure interface, thus 
avoiding deconvolution of the free-field motion down to depth. 
Non-linear  behavior  of  the  structure  may  be  modeled  by  first  carrying  out  a  static 
analysis  of  the  soil-structure  system,  and  then  carrying  out  the  transient  analysis  with 
only the structure initialized to its static state.  Because the transient analysis employs 
the dynamic scattered motion in the soil, the soil cannot have any static loads only it ― 
only  the  structure  is  subjected  to  static  forces.    Consequently,  the  structure  must  be 
supported  by  the  static  reactions  at  the  soil-structure  interface.    Additionally,  the  soil 
nodes  at  the  interface  must  be  initialized  to  be  compatible  with  the  initial  static 
displacement  of  the  structure.    LS-DYNA  will  do  these  automatically  if  the  soil-
structure  interface  is  identified  appropriately  in  the  static  analysis  and  reproduced  in 
the transient analysis.  
Thus, soil-structure interaction analysis under earthquake excitation may be carried out 
in LS-DYNA as follows: 
1.  Carry  out  a  static  analysis  of  the  soil-structure  system  (e.g.    using  dynamic 
relaxation; see *CONTROL_DYNAMIC_RELAXATION), with the soil-structure 
interface identified using *INTERFACE_SSI_STATIC_ID
Optionally,  carry  out  a  free-field  analysis  to  record  free-field  motions  on  the 
future soil-structure interface, using either *INTERFACE_SSI_AUX or *INTER-
FACE_SSI_AUX_EMBEDDED,  for  surface-supported  or  embedded  structures 
respectively.  
2.  Carry out the transient analysis as a full-deck restart job , with 
only the structure initialized to its static stress state ,  and  the  same  soil-structure  interface  identified  using  *INTERFACE_-
SSI_ID with the same ID as in static analysis: 
a)  The structure mesh must be identical to the one used for static analysis. 
b)  The soil mesh is expected to be different from the one used for static anal-
ysis, especially because non-reflecting boundary models may be used for 
transient analysis. 
c)  The meshes for the structure and the soil need not match at the interface. 
d)  Only the structure must be subjected to static loads, via *LOAD_BODY_-
PARTS 
e)  The  earthquake  ground  motion  is  specified  using  *LOAD_SEISMIC_SSI, 
and/or  read  from  motions  recorded  from  a  previous  analysis  using  *IN-
TERFACE_SSI_AUX or *INTERFACE_SSI_AUX_EMBEDDED. 
  Card 1 
Variable 
1 
ID 
Type 
I 
2 
3 
4 
5 
6 
7 
8 
HEADING 
A70 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
STRID 
SOILID 
SPR 
MPR 
Type 
I 
I 
Default 
none 
none 
I 
0 
I
Card 3 
1 
Variable 
GMSET 
Type 
I 
2 
SF 
F 
Default 
none 
1. 
*INTERFACE_SSI 
3 
4 
5 
6 
7 
8 
BIRTH 
DEATH  MEMGM 
F 
0. 
F 
I 
1028 
2500000
  VARIABLE   
DESCRIPTION
ID 
Soil-structure  interface  ID.    This  is  required  and  must  be  unique
amongst all the contact interface IDs in the model. 
HEADING 
A descriptor for the given ID. 
STRID 
Segment set ID of base of structure at soil-structure interface. 
SOILID 
Segment set ID of soil at soil-structure interface. 
SPR 
MPR 
Include  the  slave  side  in  the  *DATABASE_NCFORC  and  the 
*DATABASE_BINARY_INTFOR interface force files: 
EQ.1: slave side forces included. 
Include  the  master  side  in  the  *DATABASE_NCFORC  and  the 
*DATABASE_BINARY_INTFOR interface force files: 
EQ.1: master side forces included. 
GMSET 
Identifier  for  set  of  recorded  motions  from  *INTERFACE_SSI_-
AUX or *INTERFACE_SSI_AUX_EMBEDDED 
SF 
Recorded motion scale factor.  (default = 1.0) 
BIRTH 
Time at which specified recorded motion is activated. 
DEATH 
Time at which specified recorded motion is removed: 
EQ.0.0: default set to 1028 
MEMGM 
Size in words of buffer allocated to read in recorded motions
*INTERFACE 
1.  A  tied  contact  interface  (*CONTACT_TIED_SURFACE_TO_SURFACE)  is 
created  between  the  structure  and  the  soil  using  the  specified  segment  sets, 
with the soil segment set as the master segment set and the structure segment 
set as the slave.  Naturally, the two segment sets should not have merged nodes 
and  can  be  non-matching  in  general.    However,  the  area  covered  by  the  two 
surfaces should match.  
2.  The  options  OFFSET  and  CONSTRAINED_OFFSET  create  the  corresponding 
tied surface-to-surface contact interface. 
3.  The  soil-structure  interface  ID  is  assigned  as  the  ID  of  the  generated  contact 
interface.  
4. 
It is assumed that the soil segment set is oriented toward the structure. 
5.  Multiple soil-structure interfaces are allowed, e.g.  for bridge analysis.  
6.  The  recorded  motions  are  read  in  from  a  binary  file  named  gmbin  by  default, 
but  a  different  filename  may  be  chosen  using  the  option  GMINP  on  the  com-
mand line . 
7. 
If  the  motions  from  *INTERFACE_SSI_AUX  or  *INTERFACE_SSI_AUX_EM-
BEDDED  were  recorded  on  a  segment  set, then  the  free-field  motions  on  each 
node  in  the  master  segment  set  of  the  soil-structure  interface  are  calculated 
from the nearest segment of the segment set used to record the motions. 
If, however, the motions were recorded on a node set, then the motions on the 
master segment set nodes is found by interpolation as is done for *LOAD_SEIS-
MIC_SSI.
Available options are: 
<BLANK> 
NODE 
*INTERFACE_SSI_AUX 
Purpose:  This card records the motion at a free surface, or on a set of nodes on a free 
surface,  for  the  purpose  of  using  the  recorded  motion  as  a  free-field  motion  in  a 
subsequent  interaction  analysis  using  *INTERFACE_SSI.    By  default,  this  card  records 
motions on a segment set defining a surface, but can record motions on a node set using 
the option NODE.  Only one of *INTERFACE_SSI_AUX and *INTERFACE_SSI_AUX_-
EMBEDDED is to be used for a particular soil-structure interface.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
GMSET 
SETID 
Type 
I 
I 
Default 
none 
none 
  VARIABLE   
GMSET 
DESCRIPTION
Identifier for this set of recorded motions to be referred to in *IN-
TERFACE_SSI.  Must be unique. 
SETID 
Segment set or node set ID where motions are to be recorded. 
Remarks: 
1.  The motions on the specified segment set or node set is recorded in a binary file 
named gmbin by default, but a different filename may be chosen using option 
GMOUT on the command line . 
2.  The  output  interval  for  the  motions  may  be  specified  using  the  parameter 
GMDT on the *CONTROL_OUTPUT card, with the default value being 1/10-th 
of the output interval for D3PLOT states.
*INTERFACE_SSI_AUX_EMBEDDED_{OPTION1}_{OPTION2} 
Purpose:  This card creates a tied-contact interface and records the motions and contact 
forces  in  order  to  use  them  as  free-field  motion  and  reactions  in  a  subsequent  soil-
structure interaction analysis using *INTERFACE_SSI, where the structure is embedded 
in the soil after part of the soil has been excavated.  Only one of *INTERFACE_SSI_AUX 
and  *INTERFACE_SSI_AUX_EMBEDDED  is  to  be  used  for  a  particular  soil-structure 
interface.  
Available options for OPTION1 are: 
<BLANK> 
OFFSET 
CONSTRAINED_OFFSET 
OPTION2 allows an optional ID to be given: 
ID 
ID Card.  Additional card for ID keyword option. 
  Card 1 
Variable 
1 
ID 
Type 
I 
2 
3 
4 
5 
6 
7 
8 
HEADING 
A70 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
GMSET 
STRID 
SOILID 
SPR 
MPR 
Type 
I 
I 
I 
Default 
none 
none 
none 
I 
0 
I 
0 
DESCRIPTION
  VARIABLE   
ID 
Soil-structure  interface  ID.    This  is  required  and  must  be  unique
amongst all the contact interface IDs in the model. 
HEADING 
A descriptor for the given ID.
VARIABLE   
GMSET 
DESCRIPTION
Identifier for this set of recorded motions to be referred to in *IN-
TERFACE_SSI.  Must be unique. 
STRID 
Segment set ID at base of soil to be excavated. 
SOILID 
Segment set ID at face of rest of the soil domain. 
Include  the  slave  side  in  the  *DATABASE_NCFORC  and  the 
*DATABASE_BINARY_INTFOR interface force files: 
EQ.1: slave side forces included. 
Include  the  master  side  in  the  *DATABASE_NCFORC  and  the 
*DATABASE_BINARY_INTFOR interface force files: 
EQ.1: master side forces included. 
SPR 
MPR 
Remarks: 
1.The motions on the specified segment set or node set is recorded in a binary file 
named gmbin by default, but a different filename may be chosen using option 
GMOUT on the command line . 
2.The output interval for the motions may be specified using the parameter GMDT 
on the *CONTROL_OUTPUT card, with the default value being 1/10-th of the 
output interval for D3PLOT states.
*INTERFACE_SSI_STATIC_{OPTION}_ID 
Purpose:  This card creates a tied-contact soil-structure interface in order to record the 
static  reactions  at  the  base  of  the  structure,  which  are  to  be  used  in  a  subsequent 
dynamic  analysis  of  the  soil-structure  system  subjected  to  earthquake  excitation.    This 
card  is  intended  to  be  used  with  the  initial static  analysis  of  the  structure  subjected  to 
gravity loads. 
Available options are: 
<BLANK> 
OFFSET 
CONSTRAINED_OFFSET 
  Card 1 
Variable 
1 
ID 
Type 
I 
2 
3 
4 
5 
6 
7 
8 
HEADING 
A70 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
STRID 
SOILID 
SPR 
MPR 
Type 
I 
I 
Default 
none 
none 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
ID 
Soil-structure  interface  ID.    This  is  required  and  must  be  unique
amongst all the contact interface IDs in the model. 
HEADING 
A descriptor for the given ID. 
STRID 
Segment set ID of base of structure at soil-structure interface. 
SOILID 
Segment set ID of soil at soil-structure interface.
VARIABLE   
SPR 
DESCRIPTION
Include  the  slave  side  in  the  *DATABASE_NCFORC  and  the 
*DATABASE_BINARY_INTFOR interface force files: 
EQ.1: slave side forces included. 
MPR 
Include  the  master  side  in  the  *DATABASE_NCFORC  and  the 
*DATABASE_BINARY_INTFOR interface force files: 
EQ.1: master side forces included. 
Remarks: 
See *INTERFACE_SSI_ID.  The ID used for a particular interface in the static analysis 
must also be used for the same interface identified using *INTERFACE_SSI_ID during 
dynamic analysis.
*INTERFACE_WELDLINE_DEVELOPMENT 
Purpose:    This  keyword  causes  LS-DYNA  to  run  a  weld  line  development  calculation 
instead  of  a  finite  element  calculation.    The  input  for  this  feature  consists  of  (1)  the 
formed blank from a completed metal forming simulation, (2) the corresponding initial 
blank, and (3) if the desired weld curve on the formed blank is provided, the *INTER-
FACE_WELDLINE_DEVELOPMENT method creates a weld curve on the initial blank; 
if  the  initial  weld  curve  on  the  initial  blank  is  provided,  this  method  creates  a  weld 
curve on the final blank.  Outputs also include nodes of any element edges that intersect 
the weld curve on the initial (affectednd_i.ibo) and final blanks (affectednd_f.ibo). 
Three additional keywords must be used together (and exclusively) with this keyword.  
They are: *INITIAL_BLANK, *FINAL_PART, and *WELDING_CURVE. 
NOTE: When this card is present LS-DYNA does not proceed 
to the finite element simulation. 
Card set for *INTERFACE_WELDLINE_DEVELOPMENT. 
Development Parameter Card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IOPTION 
Type 
Default 
I 
1 
Initial Blank Card.  Following keyword *INITIAL_BLANK: 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME1 
A80 
none
Final Part Card.  Following keyword *FINAL_PART: 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME2 
A80 
none 
Welding Curve Card.  Following keyword *WELDING_CURVE: 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME3 
A80 
none 
  VARIABLE   
DESCRIPTION
IOPTION 
Welding curve development options: 
EQ.1: Calculate  initial  weld  curve  from  final  (given)  weld
curve, with output file name weldline.ibo, which will be 
on the initial blank mesh. 
EQ.-1: Calculate final  weld  curve from initial weld curve, with
output  file  name  weldline_f.ibo,  which  will  be  on  the 
formed blank mesh. 
FILENAME1 
Initial blank file name in keyword format. 
FILENAME2 
Final formed blank file name in keyword format. 
FILENAME3 
File name of the weld curve, when IOPTION: 
EQ.1: Final  (target)  welding  curve  file  name;  the  curve  is
defined using *DEFINE_CURVE_TRIM_3D. 
EQ.-1: Initial  weld  curve  file  name;  the  curve  is  defined  using
*DEFINE_CURVE_TRIM_3D.
General Remarks: 
For metal forming of tailor welded blanks, an initial straight weld line could become a 
curve on the formed part.  The amounts of deviation of the formed weld curve from its 
initial  line  depend  on  the  part  shape  and  forming  conditions.    Sometimes  the  formed 
weld curve is not desirable; so a correction to the initial weld curve is needed.  Or, given 
an initial welding curve, without performing another simulation, what would the final 
weld curve be like?  This keyword addresses these concerns. 
Mesh with adaptivity for the initial blank and final part is supported. 
Final (formed) Weld Curve: 
The final formed weld curve should be projected onto the final blank mesh if it does not 
exactly  lie  on  the  mesh  surface.    This  can  be  done  with  LS-PrePost4.2  via  the  menu 
option GeoTol → Project → Project, select Closest Projection, select Project to Elements, then 
define  the  destination  mesh  and  source  curves,  and  hit  Apply.    Sometimes  the  target 
curve  may  need  enough  points  before  projection;  the  points  may  be  added  via  menu 
option Curve → Spline → Method (Respace) → by number.  To write the curve out in *DE-
FINE_CURVE_TRIM_3D 
(To  DE-
FINE_CURVE_TRIM)  →  To  Key,  then  write  out  the  keyword  using  FILE  →  Save 
Keyword. 
format,  use  Curve  →  Convert  →  Method 
Computed Weld Curve (and IGES): 
Computed  weld  curves  are  written  with  *DEFINE_CURVE_TRIM_3D  keyword  into  a 
file  called  weldline.ibo  (or,  weldline_f.ibo,  depending  on  the  IOPTION).    The  format  of 
this  file  follows  the  keyword’s  specification.    LS-PrePost4.0  can  convert  the  computed 
curve 
under 
*INTERFACE_BLANKSIZE_DEVELOPMENT.    After  hitting  Apply,  the  curves  will 
show  up  in  the  graphics  window,  and  File  →  Save  as  →  Save  Geom  as  can  be  used  to 
write the curves out in IGES format. 
procedures 
manual 
pages 
IGES, 
see 
in 
to 
Example: 
As shown in Figure 25-41, given the initial (initialblank.k) and final blank (finalblank.k) 
configuration and a final formed weld curve (finalweldingcurve.k), the following input 
calculates a new initial weld curve on the initial blank.  In this case, the final weld curve 
is specified as straight in the drawn panel. 
*KEYWORD 
*INTERFACE_WELDLINE_DEVELOPMENT 
$OPTION 
1 
*INITIAL_BLANK
*FINAL_PART 
finalblank.k 
*WELDING_CURVE 
finalweldingcurve.k 
*END 
*INTERFACE_WELDLINE_DEVELOPMENT 
The  output  is  the  initial  weld  curve  in  the  file  weldline.ibo,  Figure  25-41.    Nodes  of 
element edges that intersect the initial weld curve are output in affectednd_i.ibo; while 
nodes  of  element  edges  that  intersect  the  final  formed  weld  curve  are  output  in 
affectednd_f.ibo, Figure 25-42. 
To  verify  the  predicted  weld  curve,  initial  blank  can  be  re-meshed  according  to  the 
curve.    A  draw  simulation  can  be  performed  again  to  confirm  the  final  weld  curve  as 
straight, Figure 25-43. 
Likewise,  if  given  an  initial  weld  curve  (initialweldingcurve.k)  and  a  final  weld  curve 
(weldline_f.ibo) can be calculated with the keyword inputs below: 
*KEYWORD 
*INTERFACE_WELDLINE_DEVELOPMENT 
$OPTION 
-1 
*INITIAL_BLANK 
initialblank.k 
*FINAL_PART 
finalblank.k 
*WELDING_CURVE 
initialweldingcurve.k 
*END
Final desired weld curve
(input: file name under 
*WELDING_CURVE)
Predicted initial weld curve
(output: weldline.ibo)
Final part
(input: file name  
under *FINAL_PART)
Initial blank
(input: file name under 
*INITIAL_BLANK)
NUMISHEET'05 Cross member
Figure 25-41.  An example for a welding curve development. 
Weld line
Sheet blank mesh
Figure 25-42.  Nodes (in green) of element edges that intersect the weld curve
are  output  in  affectednd_i.ibo  and  affectednd_f.ibo,  for  initial  and  deformed
mesh, respectively.
Remesh initial blank 
according to weldline.ibo)
Final weld curve confirms as straight
Remeshed initial blank
Final drawn part 
Figure 25-43.  Verification run 
Revision information: 
1. 
IOPTION of “1”: Revision 105189 in both double precision versions of SMP and 
MPP.   
2. 
IOPTION of “-1”: Revision 105727. 
3.  Output  of  nodes  of  element  edges  that  intersect  the  weld  curve:  Revision 
105727. 
4.  Later revisions may include improvements.
*KEYWORD_{OPTION} {memory} {memory2 = j} {NCPU = n} 
Available options include: 
<BLANK> 
ID 
JOBID 
Purpose:  The keyword, *KEYWORD, flags LS-DYNA that the input deck is a keyword 
deck rather than the structured format, which has a strictly defined format.  This must 
be the first card in the input file.  Alternatively, by typing “keyword” on the execution 
line, keyword input formats are assumed and this beginning “*KEYWORD” line is not 
required. 
There  are  3  optional  parameters  that  can  be  specified  on  the  *KEYWORD  line.    If  a 
number  {memory}  is  specified,  it  defines  the  memory  size  in  units  of  words  to  be 
allocated.    For  MPP,  if  the  parameter  {memory2 = j}  is  given,  it  defines  the  memory 
allocation  for  rest  of  the  MPP  ranks.    Note  that  if  the  memory  size  is  specified  on  the 
execution line, it will override the memory size specified on the *KEYWORD line.   
If the parameter {NCPU = n} is specified it defines the number of CPUs “n” to be used 
during the analysis.  This only applies to the Shared Memory Parallel (SMP) version of 
LS-DYNA.  For the Distributed Memory Version (MPP), the number of CPUs is always 
defined with the “mpirun” command.  Defining the number of CPUs on the execution 
line overrides what is specified on the *KEYWORD line and both override the number 
of  CPUs  specified  by  *CONTROL_PARALLEL.      An  example  of  the  {memory}  and 
{NCPU = n} options would be as follows: 
*KEYWORD 12000000 NCPU=2 
This *KEYWORD command is requesting 12 million words of memory and 2 CPUs to 
be used for the analysis with the consistency flag  turned off.  To run with the consistency flag turned on (recommended), set NCPU 
to  a  negative  value,  e.g.,  “NCPU = -2”  runs  with  2  CPUs  with  the  consistency  flag 
turned on. 
The ID and JOBID command line options are available to add a prefix to all output and 
scratch  file  names,  i.e.,  not  the  input  filenames.    This  allows  multiple  simulations  in  a 
directory since a different prefix prevents files from being overwritten.  If the ID option
characters. 
ID Card.  Additional Card  if the ID option is active.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PROJECT 
Type 
A 
NUM 
A 
Default 
none 
none 
STAGE 
A 
none 
  VARIABLE   
DESCRIPTION
PROJECT 
First part of the output file name prefix. 
NUM 
Second part of the output file name prefix. 
STAGE 
Third part of the output file name prefix. 
By using the ID option of *KEYWORD, an output file name prefix may be specified as a 
combination of   the variables PROJECT, NUM and STAGE as defined on Card 1 above.  
For example, if these variables were set literally to “PROJECT”, “NUM”, and “STAGE”, 
the first d3plot would be named: 
PROJECT_NUM_STAGE.d3plot 
Alternatively, an output file name prefix can be assigned by including “jobid=” on the 
execution line.  For example, 
lsdyna i=input.k jobid=PROJECT_NUM_STAGE 
A  third  way  to  define  an  output  file  name  prefix  is  by  using  the  JOBID  option  of  the 
*KEYWORD  command,  in  which  case  Card  1  is  defined  as  shown  below  and  the 
variable JBID acts as the output prefix.
JOBID Card.  Additional card if the JOBID option is active.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
*KEYWORD 
Variable 
Type 
Default 
JBID 
A 
none
The keyword *LOAD provides a way of defining applied forces.  The keyword control 
cards in this section are defined in alphabetical order: 
*LOAD_ALE_CONVECTION_{OPTION} 
*LOAD_BEAM_OPTION 
*LOAD_BLAST 
*LOAD_BLAST_ENHANCED 
*LOAD_BLAST_SEGMENT 
*LOAD_BLAST_SEGMENT_SET 
*LOAD_BODY_OPTION 
*LOAD_BODY_GENERALIZED 
*LOAD_BODY_POROUS 
*LOAD_BRODE 
*LOAD_DENSITY_DEPTH 
*LOAD_ERODING_PART_SET 
*LOAD_GRAVITY_PART 
*LOAD_HEAT_CONTROLLER 
*LOAD_HEAT_GENERATION_OPTION 
*LOAD_MASK 
*LOAD_MOTION_NODE 
*LOAD_MOVING_PRESSURE 
*LOAD_NODE_OPTION 
*LOAD_REMOVE_PART 
*LOAD_RIGID_BODY 
*LOAD_SEGMENT_{OPTION}
*LOAD_SEGMENT_FILE 
*LOAD_SEGMENT_FSILNK 
*LOAD_SEGMENT_NONUNIFORM_{OPTION} 
*LOAD_SEGMENT_SET_{OPTION} 
*LOAD_SEGMENT_SET_ANGLE 
*LOAD_SEGMENT_SET_NONUNIFORM_{OPTION} 
*LOAD_SEISMIC_SSI_OPTION1_{OPTION2} 
*LOAD_SHELL_{OPTION1}_{OPTION2} 
*LOAD_SPCFORC 
*LOAD_SSA 
*LOAD_STEADY_STATE_ROLLING 
*LOAD_STIFFEN_PART 
*LOAD_SUPERPLASTIC_FORMING 
*LOAD_SURFACE_STRESS_OPTION 
*LOAD_THERMAL_OPTION 
*LOAD_THERMAL_CONSTANT 
*LOAD_THERMAL_CONSTANT_ELEMENT 
*LOAD_THERMAL_CONSTANT_NODE 
*LOAD_THERMAL_D3PLOT 
*LOAD_THERMAL_LOAD_CURVE 
*LOAD_THERMAL_TOPAZ 
*LOAD_THERMAL_VARIABLE 
*LOAD_THERMAL_VARIABLE_BEAM_{OPTION} 
*LOAD_THERMAL_VARIABLE_ELEMENT_{OPTION} 
*LOAD_THERMAL_VARIABLE_NODE
*LOAD_THERMAL_VARIABLE_SHELL_{OPTION} 
*LOAD_VOLUME_LOSS
*LOAD
*LOAD_ALE_CONVECTION_{OPTION} 
Purpose:  This card is used to define the convection thermal energy transfer from a hot 
ALE  fluid  to  the  surrounding  Lagrangian  structure  (remark  1).   It  is  associated  with  a 
corresponding  coupling  card  defining  the  interaction  between  the  ALE  fluid  and  the 
Lagrangian structure.  It is only used when thermal energy transfer from the ALE fluid 
to the surrounding Lagrangian structure is significant.  This is designed specifically for 
airbag  deployment  application  where  the  heat  transfer  from  the  inflator  gas  to  the 
inflator compartment can significantly affect the inflation potential of the inflator. 
Available options include: 
<BLANK> 
ID 
To  define  an  ID  number  for  each  convection  heat  transfer  computation  in  an  optional 
card preceding all other cards for this command.  This ID number can be used to output 
the part temperature and temperature change as functions of time in the *DATABASE_-
FSI card.  To do this, set the CONVID parameter in the *DATABASE_FSI card equal to 
this ID. 
ID Card.  Additional card for ID keyword option. 
  Card 1 
Variable 
1 
ID 
Type 
I 
Default 
none 
2 
3 
4 
5 
6 
7 
8 
TITLE 
A70 
none 
Include  as  many  cards  as  necessary.    This  input  terminates  at  the  next  keyword  (“*”) 
card. 
  Card 2 
1 
2 
3 
Variable 
LAGPID 
LAGT 
LAGCP 
Type 
I 
F 
F 
4 
H 
F 
5 
6 
7 
8 
LAGMAS 
F 
Default 
none 
none 
none 
none 
none
VARIABLE   
LAGPID 
DESCRIPTION
Lagrangian  PID  (slave  PID)  from  a  corresponding  coupling  card
which receives the thermal energy in the convection heat transfer.
LAGT 
Initial temperature of this Lagrangian slave part. 
LAGCP 
H 
Constant-pressure heat capacity of this Lagrangian slave part.  It
has a per-mass unit (for example, J/[Kg*K]). 
Convection heat transfer coefficient on this Lagrangian slave part
surface.    It  is  the  amount  of  energy  (J)  transferred  per  unit  area, 
per  time,  and  per  temperature  difference.   For  example,  its  units
may be J/[m2*s*K] 
LAGMAS 
The  mass  of  the  Lagrangian  slave  part  receiving  the  thermal
energy.  This is in absolute mass unit (for example, Kg). 
Remarks: 
1.  The  only  application  of  this  card  so  far  has  been  for  the  transfer  of  thermal 
energy from the ALE hot inflator gas to the surrounding Lagrangian structure 
(inflator canister and airbag-containing compartment) in an airbag deployment 
model. 
2.  The  heat  transferred  is  taken  out  of  the  inflator  gas  thermal  energy  thus 
reducing its inflating potential.  
3.  This  is  not  a  precise  heat  transfer  modeling  attempt.    It  is  simply  one  mecha-
nism  for  taking  out  excessive  energy  from  the  inflating  potential  of  the  hot 
inflator gas. 
4.  The heat transfer formulation may roughly be represented as following.  Some 
representative units are shown just for clarity. 
[𝑄̇] = [H × 𝐴 × Δ𝑇] = (
[E]
[𝐿]2[t][T]
) × [L]2 × [T] = [Power] 
[𝑄̇] = [𝑀̇ 𝐶𝑝(𝑇Lag New − 𝑇Lag Orig)] = (
[M]
[𝑡]
) × (
[E]
[M][T]
) × [T] =
[E]
[t]
Available options include: 
ELEMENT 
SET 
*LOAD_BEAM 
Purpose:    Apply  the  distributed  traction  load  along  any  local  axis  of  beam  or  a  set  of 
beams.  The local axes are defined in Figure 27-1, see also *ELEMENT_BEAM. 
Beam Cards.  Include as many as necessary.  This input stops at the next keyword (“*”) 
card. 
5 
6 
7 
8 
Card 
1 
2 
3 
Variable 
EID/ESID 
DAL 
LCID 
Type 
I 
I 
I 
4 
SF 
F 
Default 
none 
none 
none 
1. 
  VARIABLE   
EID/ESID 
DESCRIPTION
Beam ID (EID) or beam set ID (ESID), see *ELEMENT_BEAM or 
*SET_BEAM. 
DAL = 2.  The load, as
shown, along the negative
s-axis is produced by a
positive load curve with
positive scale factor (SF). 
n1
n2
Figure 27-1.  Applied traction loads are given in force per unit length.  The s
and t directions are defined on the *ELEMENT_BEAM keyword.
DESCRIPTION
DAL 
Direction of applied load: 
EQ.1: parallel to r-axis of beam, 
EQ.2: parallel to s-axis of beam, 
EQ.3: parallel to t-axis of beam. 
*LOAD 
Load  curve  ID      or  function  ID  . 
Load  curve  scale  factor.    This  is  for  a  simple  modification  of  the
function values of the load curve. 
LCID 
SF 
Remark: 
1.The  function  defined  by  LCID  has  7  arguments:  time,  the  3  current  coordinates, 
and the 3 reference coordinates.  For example, using *DEFINE_FUNCTION, 
f(t,x,y,z,x0,y0,z0)= -10.*sqrt ( (x-x0)*(x-x0)+(y-y0)*(y-y0)+(z-z0)*(z-z0) ). 
applies a force proportional to the distance from the initial coordinates.
*LOAD_BLAST 
Purpose:    Define  an  airblast  function  for  the  application  of  pressure  loads  from  the 
detonation  of  conventional  explosives.    The  implementation  is  based  on  a  report  by 
Randers-Pehrson and Bannister [1997] where it is mentioned that this model is adequate 
for  use  in  engineering  studies  of  vehicle  responses  due  to  the  blast  from  land  mines.  
This  option  determines  the  pressure  values  when  used  in  conjunction  with  the 
keywords: *LOAD_SEGMENT, *LOAD_SEGMENT_SET, or *LOAD_SHELL. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
WGT 
XBO 
YBO 
ZBO 
TBO 
IUNIT 
ISURF 
I 
2 
6 
I 
2 
7 
8 
Type 
F 
F 
F 
F 
F 
Default 
none 
0.0 
0.0 
0.0 
0.0 
  Card 2 
1 
2 
3 
4 
5 
Variable 
CFM 
CFL 
CFT 
CFP 
DEATH 
Type 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
WGT 
Equivalent mass of TNT. 
XBO 
YBO 
ZBO 
TBO 
x-coordinate of point of explosion. 
y-coordinate of point of explosion. 
z-coordinate of point of explosion. 
Time-zero of explosion.
DESCRIPTION
IUNIT 
Unit conversion flag. 
*LOAD 
EQ.1: feet, pound-mass, seconds, psi 
EQ.2: meters, kilograms, seconds, Pascals (default) 
EQ.3: inch, dozens of slugs, seconds, psi 
EQ.4: centimeters, grams, microseconds, Megabars 
EQ.5: user conversions will be supplied  
ISURF 
Type of burst. 
EQ.1: surface  burst  -  is  located  on  or  very  near  the  ground 
surface  
EQ.2: air burst - spherical charge (default) 
CFM 
Conversion factor - pounds per LS-DYNA mass unit. 
CFL 
CFT 
CFP 
Conversion factor - feet per LS-DYNA length units. 
Conversion factor - milliseconds per LS-DYNA time unit. 
Conversion factor - psi per LS-DYNA pressure unit 
DEATH 
Death time.  Blast pressures are deactivated at this time. 
Remarks: 
1.  A  minimum  of  two  load  curves,  even  if  unreferenced,  must  be  present  in  the 
model. 
2.  Segment normals should point away from the structure and nominally toward 
the charge. 
3.  Several methods can be used to approximate the equivalent mass of TNT for a 
given  explosive.    The  simplest  involves  scaling  the  mass  by  the  ratio  of  the 
Chapman-Jouguet detonation velocities given the by relationship. 
𝑀TNT = 𝑀
𝐷𝐶𝐽2
𝐷𝐶𝐽TNT
where  MTNT  is  the  equivalent  TNT  mass  and  DCJTNT  is  the  Chapman-Jouguet 
detonation  velocity  of  TNT.    M  and  DCJ  are,  respectively,  the  mass  and  C-J 
velocity of the explosive under consideration.  “Standard” TNT is considered to 
be cast with a density of 1.57 gm/cm3 and DCJTNT = 0.693 cm/microsecond.
scaled  distance 
4.  The  empirical  equations  underlying  the  spherical  air  burst  are  valid  for  the 
range  of 
(0.147 
m/kg1/3 < Z < 40 m/kg1/3) where Z = R/M1/3, R is the distance from the charge 
center to the target and M is the TNT equivalent mass of the charge..  The range 
of  applicability  for  the  hemispherical  surface  burst  is  0.45  ft/lbm1/3 < Z < 100 
ft/lbm1/3 (0.178 m/kg1/3 < Z < 40 m/kg1/3). 
ft/lbm1/3 < Z < 100 
ft/lbm1/3 
0.37 
5.  When a charge is located on or very near the the ground surface it is considered 
to be a surface burst.  Under this circumstance the initial blast wave is immedi-
ately  reflected  and  reinforced  by  the  nearly  unyielding  ground  to  produce  a 
reflected  wave  that  moves  out  hemispherically  from  the  point  of  burst.    This 
reflected  wave  merged  with  the  initial  incident  wave  produces  overpressures 
which are greater than those produced by the initial wave alone.  In LS-DYNA 
this  wave  moves  out  spherically  from  the  burst  point  so  no  distinction  of  the 
ground orientation is made.  Target points equidistant from the burst point are 
loaded identically with the surface burst option.
*LOAD 
Purpose:    Define  an  airblast  function  for  the  application  of  pressure  loads  due  the 
detonation  of  a  conventional  explosive.    While  similar  to  *LOAD_BLAST  this  feature 
includes  enhancements  for  treating  ground-reflected  waves,  moving  warheads  and 
multiple  blast  sources.    The  loads  are  applied  to  facets  defined  with  the  keyword 
*LOAD_BLAST_SEGMENT.    A  database  containing  blast  pressure  history  is  also 
available .  
Card  Sets.    Include  as  many  sets  of  the  following  cards  as  necessary.    This  input 
terminates at the next keyword (“*”) card. 
  Card 1 
1 
Variable 
BID 
Type 
I 
2 
M 
F 
3 
4 
5 
6 
7 
8 
XBO 
YBO 
ZBO 
TBO 
UNIT 
BLAST 
F 
F 
F 
F 
Default 
none 
0.0 
0.0 
0.0 
0.0 
0.0 
Remarks 
  Card 2 
1 
1 
2 
3 
4 
5 
3 
6 
I 
2 
4 
7 
I 
2 
7 
8 
Variable 
CFM 
CFL 
CFT 
CFP 
NIDBO 
DEATH 
NEGPHS 
Type 
F 
F 
F 
F 
I 
F 
Default 
0.0 
0.0 
0.0 
0.0 
none 
1.e+20 
I 
0 
  VARIABLE   
DESCRIPTION
BID 
M 
XBO 
Blast ID.  A unique number must be defined for each blast source
(charge).  Multiple charges may be defined, however, interaction
of the waves in air is not considered. 
Equivalent mass of TNT . 
x-coordinate of charge center.
*LOAD_BLAST_ENHANCED 
DESCRIPTION
YBO 
ZBO 
TBO 
y-coordinate of charge center. 
z-coordinate of charge center. 
Time of detonation.  See Remark 3. 
UNIT 
Unit conversion flag.  See Remark 4. 
EQ.1:  pound-mass, foot,second, psi 
EQ.2:  kilogram, meter,second, Pascal (default) 
EQ.3:  dozen slugs (i.e., lbf-s2/in), inch, second, psi 
EQ.4:  centimeters, grams, microseconds, Megabars 
EQ.5:  user conversions will be supplied  
EQ.6:  kilogram, millimeter, millisecond, GPa 
EQ.7:  metric ton, millimeter, second, MPa 
EQ.8:  gram, millimeter, millisecond, MPa 
BLAST 
Type of blast source. 
EQ.1:  hemispherical  surface  burst  –  charge  is  located  on  or 
very near the ground surface  
EQ.2:  spherical  air  burst  (default)  –  no  amplification  of  the 
initial  shock  wave  due  to  interaction  with  the  ground
surface 
EQ.3:  air burst – moving non-spherical warhead 
EQ.4:  air  burst  with  ground  reflection  –  initial  shock  wave 
impinges on the ground surface and is reinforced by the
reflected wave to produce a Mach front . 
CFM 
Conversion factor - pounds per LS-DYNA mass unit. 
CFL 
CFT 
CFP 
NIDBO 
Conversion factor - feet per LS-DYNA length units. 
Conversion factor - milliseconds per LS-DYNA time unit. 
Conversion factor - psi per LS-DYNA pressure unit. 
Optional node ID representing the charge center.  If non-zero then 
XBO, YBO and XBO are ignored. 
DEATH 
Death time.  Blast pressures are deactivated at this time.
VARIABLE   
DESCRIPTION
NEGPHS 
Treatment of negative phase. 
EQ.0:  negative phase dictated by the Friedlander equation. 
EQ.1:  negative phase ignored as in ConWep. 
Moving non-spherical warhead Card.  Additional Card for BLAST = 3. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VEL 
TEMP 
RATIO 
VID 
Type 
F 
F 
F 
F 
Default 
0.0 
70.0 
1.0 
none 
  VARIABLE   
DESCRIPTION
VEL 
Speed of warhead. 
TEMP 
Ambient air temperature, Fahrenheit. 
RATIO 
Aspect  ratio  of  the  non-  spheroidal  blast  front.    This  is  the 
longitudinal    axis  radius  divided  by  the  lateral  axis  radius.
Shaped  charge  and  EFP  warheads  typically  have  significant
lateral  blast  resembling  an  oblate  spheroid  with  RATIO < 1. 
Cylindrically  cased  explosives  produce  more  blast 
in  the
longitudinal direction so RATIO > 1, rendering a prolate spheroid 
blast front, is more appropriate.. 
VID 
Vector  ID  representing  the  longitudinal  axis  of  the  warhead  .  This vector is parallel to the velocity vector
when a non-zero velocity VEL is defined.
Spherical air burst with ground reflect Card.  Additional card for BLAST = 4.  
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
GNID 
GVID 
Type 
I 
I 
Default 
none 
none 
  VARIABLE   
DESCRIPTION
ID of node residing on the ground surface. 
ID  of  vector  representing  the  vertically  upward  direction,  i.e.,
normal to the ground surface . 
GNID 
GVID 
Remarks: 
1.  Several methods can be used to approximate the equivalent mass of TNT for a 
given  explosive.    The  simplest  involves  scaling  the  mass  by  the  ratio  of  the 
Chapman-Jouguet detonation velocities given the by relationship. 
𝑀TNT = 𝑀
𝐷𝐶𝐽2
𝐷𝐶𝐽TNT
where  MTNT  is  the  equivalent  TNT  mass  and  DCJTNT  is  the  Chapman-Jouguet 
detonation  velocity  of  TNT.    M  and  DCJ  are,  respectively,  the  mass  and  C-J 
velocity of the explosive under consideration.  “Standard” TNT is considered to 
be cast with a density of 1.57 gm/cm3 and DCJTNT = 0.693 cm/microsecond. 
2.  Segment normals should point away from the structure and nominally toward 
the charge unless it is the analyst’s intent to apply pressure to the leeward side 
of a structure.  The angle of incidence is zero when the segment normal points 
directly at the charge.  Only incident pressure is applied to a segment when the 
angle of incidence is greater than 90 degrees. 
3.  The  blast  time  offset  TBO  can  be  used  to  adjust  the  detonation  time  of  the 
charge  relative  to  the  start  time  of  the  LS-DYNA  simulation.    The  detonation 
time is delayed when TBO is positive.  More commonly,  TBO is set negative so 
that the detonation occurs before time-zero of the LS-DYNA calculation.  In this 
manner, computation time is not wasted while “waiting” for the blast wave to 
reach  the  structure.    The  following  message,  written  to  the  messag  and  d3hsp 
files as well as the screen, is useful in setting TBO.
Blast wave reaches structure at 2.7832E-01 milliseconds 
As  an  example,  one  might  run  LS-DYNA  for  one  integration  cycle  and  record 
the  arrival  time  listed  in  the  message  above.    Then  TBO  is  set  to  a  negative 
number slightly smaller in magnitude than the reported arrival time, for exam-
ple  TBO = -0.275  milliseconds.    Under  this  circumstance  the  blast  wave  would 
reach the structure shortly after the start of the simulation. 
4.  Computation of blast pressure relies on an underlying method which uses base 
units  of  lbm-foot-millisecond-psi;  note  that  this  internal  unit  system  is  incon-
sistent.    Calculations  require  that  the  system  of  units  in  which  the  LS-DYNA 
model is constructed must be converted to this internal set of units.  Predefined 
and user-defined unit conversion factors are available  
and these unit conversion factors are echoed back in the d3hsp file.  Below is an 
example  of  user-defined  (UNIT = 5)  conversion  factors  for  the  gm-mm-
millisecond-Mpa unit system. 
1 = [
CFM × lb
LS-DYNA mass unit
1  = [
CFL × ft
LS-DYNA length unit
] = [ 2.2 × 10−3
⏟⏟⏟⏟⏟
= CFM
lbm
gm
] = [3.28 × 10−3 ft
mm
] 
] 
1 = [
CFT × ms
LS-DYNA time unit
] = [1.0
ms
ms
] 
1 = [
CFP × psi
LS-DYNA pressure unit
] = [145.0
psi
MPa
] 
scaled  distance 
5.  The  empirical  equations  underlying  the  spherical  air  burst  are  valid  for  the 
(0.147 
range  of 
m/kg1/3 < Z < 40 m/kg1/3) where Z = R/M1/3, R is the distance from the charge 
center to the target and M is the TNT equivalent mass of the charge.  The range 
of  applicability  for  the  hemispherical  surface  burst  is  0.45  ft/lbm1/3 < Z < 100 
ft/lbm1/3 (0.178 m/kg1/3 < Z < 40 m/kg1/3). 
ft/lbm1/3 < Z < 100 
ft/lbm1/3 
0.37 
6.  Blast loads can be used in 2D axisymmetric analyses.  Repeat the second node 
for  the  third  and  fourth  nodes  of  the  segment  definition  in  *LOAD_BLAST_-
SEGMENT and *LOAD_BLAST_SEGMENT_SET. 
7.  When a charge is located on or very near the the ground surface it is considered 
to be a surface burst.  Under this circumstance the initial blast wave is immedi-
ately  reflected  and  reinforced  by  the  nearly  unyielding  ground  to  produce  a 
reflected  hemispherical  wave  that  moves  out  from  the  point  of  burst.    This 
reflected  wave  merged  with  the  initial  incident  wave  produces  overpressures 
which are greater than those produced by the initial wave alone.  In LS-DYNA 
this  wave  moves  out  spherically  from  the  burst  point  so  no  distinction  of  the
ground orientation is made.  Target points equidistant from the burst point are 
loaded identically with the surface burst option. 
8.  The  empirical  equations  underlying  the  spherical  air  burst  with  ground 
reflection  (BLAST = 4)  are  valid  for    the  range  of  scaled  height  of  burst  1.0  
ft/lbm1/3 < Hc//M1/3 < 7.0  ft/lbm1/3  (0.397  m/kg1/3 < Z < 2.78  m/kg1/3)  where 
Hc is the height of the charge center above the ground and M is the TNT equiv-
alent mass of the charge.
F 
1. 
*LOAD_BLAST_SEGMENT 
*LOAD_BLAST_SEGMENT 
*LOAD 
Purpose:    Apply  blast  pressure  loading  over  a  triangular  or  quadrilateral  segment  for 
3D geometry or line segment for 2D geometry . 
Segment  Cards.    Include  as  many  cards  as  necessary.    This  input  ends  at  the  next 
keyword (“*”) card. 
  Card 1 
1 
Variable 
BID 
Type 
I 
2 
N1 
I 
3 
N2 
I 
4 
N3 
I 
5 
6 
7 
8 
N4 
ALEPID 
SFNRB 
SCALEP 
I 
I 
F 
Default 
none 
none 
none 
none 
none 
none 
0. 
  VARIABLE   
DESCRIPTION
BID 
Blast source ID . 
N1 
N2 
N3 
N4 
ALEPID 
SFNRB 
Node ID. 
Node ID. 
Node  ID.    For  line  segments  on  two-dimensional  geometries  set 
N3 = N2. 
Node  ID.    For  line  segments  on  two-dimensional  geometries  set 
N4 = N3 = N2 or for triangular segments in three diemensions set
N4 = N3. 
Part ID of ALE ambient part underlying this segment to be loaded
by  this  blast  .    This 
applies only when the blast load is coupled to an ALE air domain.
Scale  factor  for  the  ambient  element  non-reflecting  boundary 
condition.    Shocks  waves  reflected  back  to  the  ambient  elements
can be attenuated with this feature.  A value of 1.0 works well for
most  situations.    The  feature  is  disabled  when  a  value  of  zero  is
specified 
SCALEP 
Pressure scale factor.
*LOAD_BLAST_SEGMENT_SET 
Purpose:    Apply  blast  pressure  loading  over  each  segment  in  a  segment  set  . 
Segment Set Cards.  Include as many cards as necessary.  This input ends at the next 
keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BID 
SSID 
ALEPID 
SFNRB 
SCALEP 
Type 
I 
I 
I 
F 
Default 
none 
none 
none 
0. 
F 
1. 
  VARIABLE   
DESCRIPTION
BID 
SSID 
ALEPID 
SFNRB 
Blast source ID . 
Segment set ID . 
Part ID of ALE ambient part underlying this segment to be loaded
by  this  blast  .    This 
applies only when the blast load is coupled to an ALE air domain.
Scale  factor  for  the  ambient  element  non-reflecting  boundary 
condition.    Shocks  waves  reflected  back  to  the  ambient  elements
can be attenuated with this feature.  A value of 1.0 works well for
most situations. 
SCALEP 
Pressure scale factor. 
Remarks: 
1.  Triangular segments are defined by setting N4 = N3. 
2.  Line  segments  for  two-dimensional  geometries  are  defined  by  setting 
N4 = N3 = N2.
Available options include for base accelerations: 
*LOAD 
X 
Y 
Z 
for angular velocities: 
RX 
RY 
RZ 
for loading in any direction, specified by vector components: 
VECTOR  
and to specify a part set: 
PARTS 
Purpose:    Define  body  force  loads  due  to  a  prescribed  base  acceleration  or  angular 
velocity using global axes directions.  This option applies nodal forces only: it cannot be 
used to prescribe translational or rotational motion.  These body forces do not take into 
account non-physical mass added via mass scaling; see *CONTROL_TIMESTEP. 
NOTE:  This data applies to all nodes in the complete prob-
lem  unless  a  part  subset  is  specified  via  the 
*LOAD_BODY_PARTS keyword. 
If  a  part  subset  with  *LOAD_BODY_PARTS  then  all  nodal  points  belonging  to  the 
subset will have body forces applied. 
NOTE:  Only  one  *LOAD_BODY_PARTS  card  is  permitted 
per deck.  To specify, for instance, one body load on 
one part and another body load on another part use 
*LOAD_BODY_GENERALIZED instead.
For options X, Y, Z, RX, RY, RZ and VECTOR. 
  Card 1 
1 
Variable 
LCID 
Type 
I 
2 
SF 
F 
Default 
none 
1. 
3 
4 
LCIDDR 
XC 
I 
0 
F 
0. 
8 
5 
YC 
F 
0. 
6 
ZC 
F 
0. 
7 
CID 
I 
0 
For option PARTS.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PSID 
Type 
I 
Default 
none 
For option VECTOR.  
  Card 2 
Variable 
1 
V1 
Type 
F 
2 
V2 
F 
3 
V3 
F 
Default 
0.0 
0.0 
0.0 
4 
5 
6 
7 
8 
  VARIABLE   
DESCRIPTION
LCID 
Load curve ID, see *DEFINE_CURVE. 
SF 
Load curve scale factor
LCIDDR 
XC 
YC 
ZC 
CID 
*LOAD 
DESCRIPTION
Load  curve  ID  for  dynamic  relaxation  phase  (optional).    This  is
needed  when  dynamic  relaxation  is  defined  and  a  different  load
curve  to  LCID  is  required  during  the  dynamic  relaxation  phase.
Note  if  LCID  is  undefined  then  no  body  load  will  be  applied
during dynamic relaxation regardless of the value LCIDDR.  See 
*CONTROL_DYNAMIC_RELAXATION 
𝑥-center of rotation, define for angular velocities. 
𝑦-center of rotation, define for angular velocities. 
𝑧-center of rotation, define for angular velocities. 
Coordinate  system  ID  to  define  acceleration  in  local  coordinate
system.  The accelerations (LCID) are with respect to CID. 
EQ.0: global 
PSID 
Part set ID. 
V1, V2, V3 
Vector components of vector 𝐕. 
General remarks: 
Translational  base  accelerations  allow  body  force  loads  to  be  imposed  on  a  structure.  
Conceptually, base acceleration may be thought of as accelerating the coordinate system 
in  the  direction  specified,  and,  thus,  the  inertial  loads  acting  on  the  model  are  of 
opposite sign.  For example, if a cylinder were fixed to the 𝑦-𝑧 plane and extended in the 
positive x-direction, then a positive 𝑥-direction base acceleration would tend to shorten 
the cylinder, i.e., create forces acting in the negative 𝑥-direction. 
Base  accelerations  are  frequently  used  to  impose  gravitational  loads  during  dynamic 
relaxation to initialize the stresses and displacements.  During the analysis, in this latter 
case,  the  body  forces  loads  are  held  constant  to  simulate  gravitational  loads.    When 
imposing  loads  during  dynamic  relaxation,  it  is  recommended  that  the  load  curve 
slowly ramp up to avoid the excitation of a high frequency response. 
Body force loads due to the angular velocity about an axis are calculated with respect to 
the  deformed  configuration  and  act  radially  outward  from  the  axis  of  rotation.  
Torsional  effects  which  arise  from  changes  in  angular  velocity  are  neglected  with  this 
option.  The angular velocity is assumed to have the units of radians per unit time. 
The body force density is given at a point 𝐏 of the body by:
(0.0,0.0,0.0)
(0.0,0.0,0.0)
Initial configuration
Gravity-loaded shape
Figure 27-2.  A validation example for option VECTOR. 
𝐛 = 𝜌[𝛚 × (𝛚 × 𝐫)] 
where 𝜌 is the mass density, 𝛚 is the angular velocity vector, and 𝐫 is a position vector 
from  the  origin  to  point  𝐏.    Although  the  angular  velocity  may  vary  with  time,  the 
effects of angular acceleration are not included. 
Angular  velocities  are  useful  for  studying  transient  deformation  of  spinning  three-
dimensional  objects.    Typical  applications  have  included  stress  initialization  during 
dynamic relaxation where the initial rotational velocities are assigned at the completion 
of the initialization, and this option ceases to be active. 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *LOAD_BODY_Z 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Add gravity such that it acts in the negative Z-direction. 
$  Use units of mm/ms2.  Since gravity is constant, the load 
$  curve is set as a constant equal to 1.  If the simulation 
$  is to exceed 1000 ms, then the load curve needs to be 
$  extended. 
$ 
$$$  Note: Positive body load acts in the negative direction. 
$ 
*LOAD_BODY_Z 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$     lcid        sf    lciddr        xc        yc        zc 
         5   0.00981 
$ 
$ 
*DEFINE_CURVE 
$     lcid      sidr      scla      sclo      offa      offo 
         5
$ 
$           abscissa            ordinate 
                0.00               1.000 
             1000.00               1.000 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
About option VECTOR: 
The  vector  V  defines  the  direction  of  the  body  force.    Body  forces  act  in  the  negative 
direction of the vector V. 
In  an  example  shown  in  Figure  27-2,  a  rectangular  sheet  metal  blank  is  loaded  with 
gravity  into  a  ball  defined  as  a  fixed  rigid  body.    Given  the  global  coordinate  system 
shown, if the part set ID of the blank is 1, the keywords responsible for specifying the 
body force (in units of mm, second, tonne and Newton) in positive direction of (1.0, 1.0, 
1.0) will be as follows, 
*LOAD_BODY_PARTS 
1 
*LOAD_BODY_VECTOR 
101, 9810.0 
-1.0, -1.0, -1.0 
*DEFINE_CURVE 
101 
0.0, 1.0 
10.0, 1.0 
It is note that straight lines represent a cube with each edge length of 500.0mm. 
Revision information: 
The_VECTOR option is available in LS-DYNA R5 Revision 59290 and later releases.
*LOAD_BODY_GENERALIZED_OPTION 
Available options include: 
SET_NODE 
SET_PART 
Purpose:  Define body force loads due to a prescribed base acceleration or a prescribed 
angular motion over a subset of the complete problem.  The subset is defined by using 
nodes or parts.  Warning: Nodes, which belong to rigid bodies, should not be specified.  
Rigid bodies must be included within the part sets definitions.  
The  body  forces  defined  using  this  command  do  not  take  into  account  non-physical 
mass added via mass scaling; see *CONTROL_TIMESTEP. 
Card Sets.  Include as many sets of Cards 1 and 2 as necessary.  This input terminates 
at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
Variable 
N1/SID 
N2/0 
LCID 
DRLCID 
XC 
Type 
I 
I 
I 
Default 
none 
none 
none 
I 
0 
F 
0. 
8 
6 
YC 
F 
0. 
7 
ZC 
F 
0. 
Remarks 
  Card 2 
Variable 
1 
AX 
Type 
F 
Default 
0. 
2 
AY 
F 
0. 
3 
AZ 
F 
0. 
4 
5 
6 
7 
8 
OMX 
OMY 
OMZ 
CID 
ANGTYP 
F 
0. 
F 
0. 
F 
0. 
I 
0 
A 
CENT 
Remarks 
1, 2 
1, 2 
1, 2 
3, 4, 5 
3, 4, 5 
3, 4, 5  optional
VARIABLE   
DESCRIPTION
N1/SID 
Beginning node ID for body force load or the node or part set ID. 
N2 
Ending  node  ID  for  body  force  load.    Set  to  zero  if  a  set  ID  is
defined. 
LCID 
Load curve ID, see *DEFINE_CURVE. 
DRLCID 
Load  curve  ID  for  dynamic  relaxation  phase.    Only  necessary  if
dynamic  relaxation  is defined.    See  *CONTROL_DYNAMIC_RE-
LAXATION. 
XC 
YC 
ZC 
AX 
AY 
AZ 
OMX 
OMY 
OMZ 
CID 
𝑥-center of rotation.  Define only for angular motion. 
𝑦-center of rotation.  Define only for angular motion. 
𝑧-center of rotation.  Define only for angular motion. 
Scale factor for acceleration in 𝑥-direction 
Scale factor for acceleration in 𝑦-direction 
Scale factor for acceleration in 𝑧-direction 
Scale factor for 𝑥-angular velocity or acceleration 
Scale factor for 𝑦-angular velocity or acceleration 
Scale factor for 𝑧-angular velocity or acceleration 
Coordinate  system  ID  to  define  acceleration 
local
coordinate system.  The coordinate (XC, YC, ZC) is defined with
respect  to  the  local  coordinate  system  if  CID  is  nonzero.    The
accelerations,  LCID  and  their  scale  factors  are  with  respect  to 
CID. 
in  the 
EQ.0: global
*LOAD_BODY_GENERALIZED 
DESCRIPTION
ANGTYP 
Type of body loads due to angular motion 
EQ.CENT:  body load from centrifugal acceleration, 
𝜌[𝛚 × (𝛚 × 𝐫)]. 
EQ.CORI:  body load from Coriolis-type acceleration, 
EQ.ROTA:  body load from rotational acceleration, 
2𝜌(𝛚 × 𝐯). 
𝜌(𝛂 × 𝐫), 
where  𝛚  is  the  angular  velocity,  𝛂  is  the  angular 
acceleration, 𝐫 is the position vector relative to cen-
ter of rotation and 𝐯 is the velocity vector 
Remarks: 
1.  Translational  base  accelerations  allow  body  forces  loads  to  be  imposed  on  a 
structure.  Conceptually, base acceleration may be thought of as accelerating the 
coordinate system in the direction specified, and, thus, the inertial loads acting 
on the model are of opposite sign.  For example, if a cylinder were fixed to the 
y-z  plane  and  extended  in  the  positive  x-direction,  then  a  positive  x-direction 
base acceleration would tend to shorten the cylinder, i.e., create forces acting in 
the negative x-direction. 
2.  Base  accelerations  are  frequently  used  to  impose  gravitational  loads  during 
dynamic  relaxation  to  initialize  the  stresses  and  displacements.    During  the 
analysis, in this latter case, the body forces loads are held constant to simulate 
gravitational  loads.    When  imposing  loads  during  dynamic  relaxation,  it  is 
recommended that the load curve slowly ramp up to avoid the excitation of a 
high frequency response. 
3.  Body  force  loads  due  to  the  angular  motion  about  an  axis  are  calculated  with 
respect  to  the  deformed  configuration.    When  ANGYP = CENT  or  CORI,  tor-
sional effects which arise from changes in angular velocity are neglected.  Such 
torsional  effects  can  be  taken  into  account  by  setting  ANGTYP = ROTA.    The 
angular velocity is assumed to have the units of radians per unit time, accord-
ingly angular acceleration has the units of radians/time2. 
4.  The body force density is given at a point 𝐏 of the body by: 
𝒃 = 𝜌[𝛚 × (𝛚 × 𝐫)]
where 𝜌 is the mass density, 𝛚 is the angular velocity vector, and 𝐫 is a position 
vector from the origin to point 𝐏.  Although the angular velocity may vary with 
time, the effects of angular acceleration are included. 
5.  Angular  velocities  are  useful  for  studying  transient  deformation  of  spinning 
three-dimensional objects.  Typical applications have included stress initializa-
tion  during  dynamic  relaxation  where  the  initial  rotational  velocities  are  as-
signed at the completion of the initialization, and this option ceases to be active.
*LOAD_BODY_POROUS 
Purpose:  Define the effects of porosity on the flow with body-force-like loads applied 
to the ALE element nodes.  Ergun porous flow assumptions are used.  This only applies 
to non-deformable (constant-porosity), fully saturated porous media.  This model only 
works with a non-zero and constant viscosity fluid defined via either *MAT_NULL or 
*MAT_ALE_VISCOUS card. 
Card Sets.  Include as many sets of Cards 1 and 2 as necessary.  This input terminates 
at the next keyword (“*”) card. 
3 
AX 
F 
4 
AY 
F 
5 
AZ 
F 
6 
BX 
F 
7 
BY 
F 
8 
BZ 
F 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
3 
4 
5 
6 
7 
8 
  Card 1 
1 
2 
Variable 
SID 
SIDTYP 
I 
0 
2 
Type 
Default 
I 
0 
  Card 2 
1 
Variable 
AOPT 
Type 
Default 
I 
0 
  VARIABLE   
DESCRIPTION
SID 
Set ID of the ALE fluid part subjected to porous flow condition. 
SIDTYP 
Set  ID  type  of  the  SID  above.    If  SIDTYP = 0  (default),  then  the 
SID = PSID (part set ID).  If SIDTYP = 1, then SID = PID (part ID).
AX, AY, AZ 
Viscous  coefficients  for  viscous  terms  in  global  𝑥,  𝑦,  and  𝑧
directions (please see equation below).  If 𝐴𝑥 ≠ 0 and 𝐴𝑦 = 𝐴𝑧 = 0
then  an  isotropic  viscous  permeability  condition  is  assumed  for
the porous medium.
VARIABLE   
BX, BY, BZ 
DESCRIPTION
Inertial coefficients for inertia terms in global 𝑥, 𝑦, and 𝑧 directions 
(please  see  equation  below).    If  𝐵𝑥 ≠ 0,  and  𝐵𝑦 = 𝐵𝑧 = 0  then  an 
isotropic  inertial  permeability  condition  is  assumed  for  the
porous medium. 
AOPT 
Material axis option: 
EQ.0: 
inactive. 
EQ.1:  The forces are applied in a local system attached to the
ALE  solid    . 
Remarks: 
1.  Consider the basic general Ergun equation for porous flow in one direction: 
Δ𝑃
Δ𝐿
=
𝑘1
𝑉𝑠 +
𝑘2
2 
𝑉𝑠
Where 
𝜌 = Fluid Density 
𝜇 = Fluid dynamic vicosity 
𝑉𝑠 =
4𝑄
𝜋𝐷2 = Superficial fluid velocity 
𝑄 = Overall volume flow rate  (
m3
) 
𝐷 = Porous channel characteristic width (perpendicular to ΔL) 
𝜀3𝑑𝑝
𝑘1 =
150(1 − 𝜀)2 = Permeability parameter 
𝑘2 =
𝜀3𝑑𝑝
1.75(1 − 𝜀)
= Passability parameter 
𝜖 = Porosity=
total pore volume
total media volume
𝑑𝑝 = Effective particle diameter 
2.  The  above  equation  can  be  generalized  into  3  dimensional  flows  where  each 
component may be written as 
−
𝑑𝑃
𝑑𝑥𝑖
= 𝐴𝑖𝜇𝑉𝑖 + 𝐵𝑖𝜌|𝑉𝑖|𝑉𝑖
where 𝑖 = 1,2,3 refers to the global coordinate directions (no summation intend-
ed for repeated indices), 𝜇 is the constant dynamic viscosity, 𝜌 is the fluid densi-
ty,  𝑉𝑖  is  the  fluid  velocity  components,  𝐴𝑖  is  analogous  to  𝑘1  above,  and    𝐵𝑖  is 
analogous to 𝑘2 above.  A matrix version can be defined by ALE elements with 
*DEFINE_POROUS_ALE. 
3. 
If 𝐵𝑖 = 0, the equation is reduced to simple Darcy Law for porous flow (may be 
good  for  sand-like  flow).    For  coarse  grain  (rocks)  media,  the  inertia  term  will 
be important and the user needs to input these coefficients.
*LOAD 
Purpose:  Define Brode function for application of pressure loads due to explosion, see 
Brode [1970], also see *LOAD_SEGMENT, *LOAD_SEGMENT_SET, or *LOAD_SHELL. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
YLD 
BHT 
XBO 
YBO 
ZBO 
TBO 
TALC 
SFLC 
Type 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Remarks 
  Card 2 
1 
2 
3 
4 
5 
6 
I 
0 
1 
7 
I 
0 
1 
8 
Variable 
CFL 
CFT 
CFP 
Type 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
YLD 
BHT 
XBO 
YBO 
ZBO 
TBO 
TALC 
Yield (Kt, equivalent tons of TNT). 
Height of burst. 
x-coordinates of Brode origin. 
y-coordinates of Brode origin. 
z-coordinates of Brode origin. 
Time offset of Brode origin. 
Load curve number giving time of arrival versus range relative to 
Brode  origin  (space,  time),  see  *DEFINE_CURVE  and  remark 
below.
Load curve number giving yield scaling versus scaled time (time
relative  to  Brode  origin  divided  by  [yield(**1⁄3)])  origin  (space, 
time), see *DEFINE_CURVE and remark below. 
Conversion factor - kft to LS-DYNA length units. 
Conversion factor - milliseconds to LS-DYNA time units. 
Conversion factor - psi to LS-DYNA pressure units. 
*LOAD 
  VARIABLE   
SFLC 
CFL 
CFT 
CFP 
Remarks: 
1. 
If these curves are defined a variable yield is assumed.  Both load curves must 
be specified for the variable yield option.  If this option is used, the shock time 
of arrival is found from the time of arrival curve.  The yield used in the Brode 
formulas  is  computed  by  taking  the  value  from  the  yield  scaling  curve  at  the 
current time/[yield(**1⁄3)] and multiplying that value by yield.
*LOAD 
Purpose:    Define  density  versus  depth  for  gravity  loading.    This  option  has  been 
occasionally  used  for  analyzing  underground  and  submerged  structures  where  the 
gravitational  preload  is  important.    The  purpose  of  this  option  is  to  initialize  the 
hydrostatic pressure field at the integration points in the element. 
This card should be only defined once in the input deck. 
  Card 1 
1 
Variable 
PSID 
Type 
Default 
I 
0 
Remarks 
1,2 
2 
GC 
F 
0.0 
3 
4 
5 
6 
7 
8 
DIR 
LCID 
I 
1 
I 
none 
3 
  VARIABLE   
DESCRIPTION
PSID 
GC 
DIR 
Part set ID, see *SET_PART.  If a PSID of zero is defined then all 
parts are initialized. 
Gravitational acceleration value. 
Direction of loading: 
EQ.1: global x, 
EQ.2: global y, 
EQ.3: global z. 
LCID 
Load  curve  ID  defining  density  versus  depth,  see  *DEFINE_-
CURVE. 
Remarks: 
1.  Density  versus  depth  curves  are  used  to  initialize  hydrostatic  pressure  due  to 
gravity acting on an overburden material.  The hydrostatic pressure acting at a 
material point at depth, d, is given by:
𝑑surface
𝑝 = − ∫ 𝜌(𝑧)𝑔𝑑𝑧
where    𝑝  is  pressure,  𝑑surface,  is  the  depth  of  the  surface  of  the  material  to  be 
initialized (usually zero), 𝜌 (𝑧) is the mass density at depth 𝑧, and 𝑔 is the accel-
eration of gravity.  This integral is evaluated for each integration point.  Depth 
may be measured along any of the global coordinate axes, and the sign conven-
tion of the global coordinate system should be respected.  The sign convention 
of gravity also follows that of the global coordinate system.  For example, if the 
positive 𝑧 axis points "up", then gravitational acceleration should be input as a 
negative number. 
2.  For this option there is a limit of 12 parts that can be defined by PSID, unless all 
parts are initialized. 
3.  Depth  is  the  ordinate  of  the  curve  and  is  input  as  a  descending  x,  y,  or  z 
coordinate value.  Density is the abscissa of the curve and must vary (increase) 
with depth, i.e., an infinite slope is not allowed. 
4.  See also GRAV in *PART.
*LOAD 
Purpose:  Apply a pressure load to the exposed surface composed of solid elements that 
may erode. 
Card Sets.  Include as many sets of Cards 1 and 2 as necessary.  This input terminates 
at the next keyword (“*”) card. 
Card 
Variable 
1 
ID 
2 
LCID 
Type 
I 
I 
Default 
none 
none 
  Card 2 
1 
Variable 
IFLAG 
Type 
Default 
I 
0 
2 
X 
F 
5 
6 
7 
8 
PSID 
BOXID 
MEM 
ALPHA 
I 
0 
6 
I 
F 
50 
80 
7 
8 
3 
SF 
F 
1 
3 
Y 
F 
4 
AT 
F 
I 
0.0 
none 
4 
Z 
F 
5 
BETA 
F 
0.0 
0.0 
0.0 
90 
  VARIABLE   
DESCRIPTION
ID 
LCID 
SF 
AT 
ID number. 
Load  curve  ID  defining  pressure  as  a  function  of  time,  see  *DE-
FINE_CURVE. 
Scale factor. 
Arrival time. 
PSID 
Part set ID, see *SET_PART. 
BOXID 
Box  ID,  see  *DEFINE_BOX.    Any  segment  that  would  otherwise 
be  loaded  but  whose  centroid  falls  outside  of  this  box  is  not
loaded.
MEM 
ALPHA 
IFLAG 
*LOAD_ERODING_PART_SET 
DESCRIPTION
Extra  memory,  in  percent,  to  be  allocated  above  the  initial
memory  for  storing  the  new  load  segments  exposed  by  the
erosion. 
The  maximum  angle  (in  degrees)  permitted  between  the  normal
of a segment at its centroid and the average normal at its nodes. 
This angle is used to eliminate interior segments. 
Flag for choosing a subset of the exposed surface that is oriented
towards  a  blast  or  other  loading  source.    The  vector  from  the
center  of  the  element  to  the  source  location  must  be  within  an
angle  of  BETA  of  the  surface  normal.    If  IFLAG >  0,  then  the 
subset  is  chosen,  otherwise  if  IFLAG = 0,  the  entire  surface  is 
loaded. 
X, Y, Z 
Optional source location. 
BETA 
Maximum  permitted  angle  (in  degrees)  between  the  surface
normal and the vector to the source.  The exposed segment is not 
loaded if the calculated angle is greater than BETA. 
Remarks: 
1. 
2. 
If LCID is input as -1, then the Brode function is used to determine the pressure 
for the segments, see *LOAD_BRODE. 
If LCID is input as -2, then an empirical air blast function is used to determine 
the pressure for the segments, see *LOAD_BLAST. 
3.  The  load  curve  multipliers  may  be  used  to  increase  or  decrease  the  pressure.  
The time value is not scaled. 
4.  The activation time, AT, is the time during the solution that the pressure begins 
to act.  Until this time, the pressure is ignored.  The function value of the load 
curves  will  be  evaluated  at  the  offset  time  given  by  the  difference  of  the  solu-
tion time and AT i.e., (solution time-AT). 
5.  For  proper  evolution of  the  loaded  surface, it  is  a  requirement  that  DTMIN  in 
*CONTROL_TERMINATION  be  greater  trhan  zero  and  ERODE  in  *CON-
TROL_TIMESTEP be set to 1.
Available options are: 
<BLANK> 
SET 
*LOAD 
Purpose:    Define  gravity  for  individual  parts.    This  feature  is  intended  for  use  with 
*LOAD_STIFFEN_PART to simulate staged construction.  This keyword is available for 
solids and shells, and also beam element types 1, 2, 6, and 9.  It is not currently available 
for thick shells. 
Part Cards.  Include this card as many times as necessary.  This input ends at the next 
keyword (“*”) card. 
  Card 1 
1 
2 
Variable 
PID 
DOF 
Type 
I 
I 
3 
LC 
I 
Default 
none 
none 
none 
4 
5 
6 
7 
8 
ACCEL 
LCDR 
STGA 
STGR 
F 
0 
I 
none 
I 
0 
I 
0 
DESCRIPTION
  VARIABLE   
PID/PSID 
DOF 
LC 
Part  ID  (or  Part  Set  ID  for  the_SET  option)  for  application  of 
gravity load 
Direction: enter 1, 2 or 3 for 𝑥, 𝑦 or 𝑧 
Load  curve  defining  factor  vs.    time  (or  zero  if  STGA,  STGR  are
defined) 
ACCEL 
Acceleration (will be multiplied by factor from curve 
Load curve defining factor vs.  time during dynamic relaxation 
Construction stage at which part is added (optional) 
Construction stage at which part is removed (optional) 
LCDR 
STGA 
STGR 
Remarks: 
1.  There are 3 options for defining how the gravity load on a part varies with time.
a)  Curve LC gives factor vs time.  This overrides the other methods if LC is 
non-zero. 
b)  STGA,  STGR  refer  to  stages  at  which  part  is  added  and  removed  –  the 
stages  are  defined  in  *DEFINE_CONSTRUCTION_STAGES.    If  STGA  is 
zero, the gravity load starts at time zero.  If not, it ramps up from the small 
factor FACT (on *CONTROL_STAGED_CONSTRUCTION) up to full val-
ue  over  the  ramp  time  at  the  start  of  stage  STGA.    If  STGR  is  zero,  the 
gravity load continues until the end of the analysis.  If not, it ramps down 
from full value to FACT over the ramp time at the start of stage STGR. 
c)  *DEFINE_STAGED_CONSTRUCTION_PART  can  be  used  instead  of 
*LOAD_GRAVITY_PART  to  define  this  loading.    During  initialization,  a 
LOAD_GRAVITY_PART card will be created and the effect is the same as 
using  the  STGA,  STGR  method  described  above;  ACCEL  is  then  taken 
from *CONTROL_STAGED_CONSTRUCTION. 
2.  This  feature  calculates  the  loading  from  the  mass  of  the  elements  of  the 
referenced  parts  only  (density × volume).    This  mass  does  not  include  any  at-
tached  lumped  mass  elements.    Only  solid,  beam  and  shell  elements  can  be 
loaded.
*LOAD 
Purpose:    Used  to  define  a  thermostat  control  function.    The  thermostat  controls  the 
heat generation within a material by monitoring a remote nodal temperature.  Control 
can be specified as on-off, proportional, integral, or proportional with integral. 
Sensor Node Cards.  Include up to 20 cards.  This input ends at the next keyword (“*”) 
card. 
  Card 1 
1 
2 
3 
4 
5 
Variable 
NODE 
PID 
LOAD 
TSET 
TYPE 
Type 
I 
I 
F 
F 
I 
8 
6 
GP 
F 
7 
GI 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
NODE 
Sensor is located at this node number. 
PID 
LOAD 
TSET 
Part  ID  assigned  to  the  elements  modeling  the  heater  or  cooler
being controlled.   
Heater output 𝑞0.  [typical units: W/m3] 
Controller  set  point  temperature  at  the  location  identified  by
NODE. 
TYPE 
Type of control function. 
EQ.1: on-off 
EQ.2: proportional + integral 
GP 
GI 
Proportional gain. 
Integral gain. 
Remarks: 
The thermostat control function is 
𝑞 ̇′′′ = 𝑞 ̇0
′′′ [𝐺𝑃(𝑇set − 𝑇node) + 𝐺𝐼 ∫ (𝑇set − 𝑇node)
𝑑𝑡]
𝑡=0
*LOAD_HEAT_GENERATION_OPTION 
Available options include: 
SOLID 
SET_SOLID 
SHELL 
SET_SHELL 
Purpose:  Define elements or element sets with heat generation. 
Generation  Cards.    Include  as  many  cards  as  necessary.    This  input  ends  at  the  next 
keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
LCID 
MULT 
WBLCID 
CBLCID 
TBLCID 
Type 
I 
I 
F 
Default 
none 
none 
0. 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
SID 
LCID 
Element ID or element set ID, see *ELEMENT_SOLID, *SET_SOL-
ID, *ELEMENT_SHELL, and *SET_SHELL, respectively. 
Volumetric  heat  generation  rate, 𝑞 ̇′′′,  specification.    SI  units  are 
W/m3.    This  parameter  can  reference  a  load  curve  ID    or  a  function  ID  .    When  the  reference  is  to  a  curve,  LCID  has  the
following interpretation: 
GT.0:  𝑞 ̇′′′  is  defined  by  a  curve  consisting  of  (time,  𝑞 ̇′′′)  data 
pairs. 
EQ.0: 𝑞 ̇′′′ is a constant defined by the value MULT. 
LT.0:  𝑞 ̇′′′ is defined by a curve consisting of (temperature, 𝑞 ̇′′′) 
data  pairs.    Enter  |-LCID|  on  the  DEFINE_CURVE 
keyword. 
MULT 
Volumetric heat generation, 𝑞̇′′′, curve multiplier.
DESCRIPTION
Load curve ID defining the blood perfusion rate [e.g., kg/m3 sec] 
as a function of time. 
Load curve ID defining the blood specific heat [e.g., J/kg C] as a
function of the blood temperature. 
Load  curve  ID  defining  the  blood  temperature  [e.g.,  C]  as  a
function of time. 
  VARIABLE   
WBLCID 
CBLCID 
TBLCID 
Remarks: 
1. 
If  LCID  references  a  DEFINE_FUNCTION,  the  following  function  arguments 
are allowed 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑇, 𝑡)where: 
𝑥, 𝑦, 𝑧 = element centroid coordinates 
𝑣𝑥, 𝑣𝑦, 𝑣𝑧 = element centroid velocity components 
𝑇 = element integration point temperature 
𝑡 = solution time 
2.  Rate of heat transfer from blood to tissue  = 𝑊𝑏𝐶𝑏(𝑇𝑏 − 𝑇) [units: J/m3 sec]
*LOAD_MASK 
Purpose:    Apply  a  distributed  pressure  load  over  a  three-dimensional  shell  part.    The 
pressure  is  applied  to  a  subset  of  elements  that  are  within  a  fixed  global  box  and  lie 
either outside or inside of a closed curve in space which is projected onto the surface. 
Card Sets.  Include as many sets of Cards 1 and 2 as necessary.  This input terminates 
at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
LCID 
VID1 
OFF 
BOXID 
LCIDM 
VID2 
INOUT 
Type 
I 
I 
F 
Default 
none 
none 
1. 
F 
0. 
I 
0 
I 
0 
I 
none 
I 
0 
4 
5 
6 
7 
8 
Remarks 
1 
  Card 2 
1 
2 
Variable 
ICYCLE 
2 
3 
Type 
I 
Default 
200 
Remarks 
  VARIABLE   
DESCRIPTION
PID 
LCID 
Part ID (PID).  This part must consist of 3D shell elements.  To use
this  option  with  solid  element  the  surface  of  the  solid  elements
must be covered with null shells.  See *MAT_NULL. 
Curve  ID  defining  the  pressure  time  history,  see  *DEFINE_-
CURVE.
VID1 
OFF 
BOXID 
LCIDM 
VID2 
INOUT 
ICYCLE 
*LOAD 
DESCRIPTION
Vector  ID  normal  to  the  surface  on  which  the  applied  pressure
acts.    Positive  pressure  acts  in  a  direction  that  is  in  the  opposite
direction.    This  vector  may  be  used  if  the  surface  on  which  the
pressure acts is relatively flat.  If zero, the pressure load depends 
on the orientation of the shell elements as shown in Figure 27-4. 
Pressure loads will be discontinued if  ∣𝑉𝐼𝐷1 ⋅ 𝑛𝑠ℎ𝑒𝑙𝑙∣ < 𝑂𝐹𝐹 where 
𝑛𝑠ℎ𝑒𝑙𝑙 is the normal vector to the shell element. 
Only elements inside the box with part ID, PID, are considered.  If
no  ID  is  given  all  elements  of  part  ID,  PID,  are  included.    When
the  active  list  of  elements  are  updated,  elements  outside  the  box
the  current 
will  no 
configuration is always used. 
longer  have  pressure  applied, 
i.e., 
Curve ID defining the mask.  This curve gives (x,y) pairs of points
in  a  local  coordinate  system  defined  by  the  vector  ID,  VID2.
Generally, the curve should form a closed loop, i.e., the first point 
is identical to the last point, and the curve should be flagged as a
DATTYP = 1 curve in the *DEFINE_CURVE section.   If no curve 
ID  is  given,  all  elements  of  part  ID,  PID,  are  included  with  the
exception  of  those  deleted  by  the  box.    The  mask  works  like  the 
and 
trimming  option, 
Figure15-18. 
see  DEFINE_CURVE_TRIM 
i.e., 
Vector  ID  used  to  project  the  masking  curve  onto  the  surface  of
part  ID,  PID.    The  origin  of  this  vector  determines  the  origin  of
the  local  system  that  the  coordinates  of  the  PID  are  transformed
into  prior  to  determining  the  pressure  distribution  in  the  local
system.    This  curve  must  be  defined  if  LCIDM  is  nonzero.    See
Figure15-18. 
If  0,  elements  whose  center  falls  inside  the  projected  curve  are 
considered.  If 1, elements whose center falls outside the projected
curve are considered. 
Number  of  time  steps  between  updating  the  list  of  active
elements  (default = 200).    The  list  update  can  be  quite  expensive 
and should be done at a reasonable interval.  The default is not be
appropriate for all problems.
1.  The part ID must consist of 3D shell elements.
*LOAD_MASK
*LOAD 
Purpose:  Apply a concentrated nodal force or moment to a node based on the motion 
of another node. 
Node Cards.  This input continues until the next keyword (“*”) card. 
Card 
1 
2 
3 
Variable 
NODE1 
DOF1 
LCID 
Type 
I 
I 
I 
4 
SF 
F 
Default 
none 
none 
none 
1. 
Remarks 
5 
6 
7 
8 
CID1 
NODE2 
DOF2 
CID2 
I 
0 
1 
I 
0 
I 
0 
I 
0 
1 
  VARIABLE   
DESCRIPTION
NODE1 
Node ID for the concentrated force. 
DOF1 
Applicable degrees-of-freedom: 
EQ.1: x-direction of load action, 
EQ.2: y-direction of load action, 
EQ.3: z-direction of load action, 
EQ.4: moment about the x-axis, 
EQ.5: moment about the y-axis, 
EQ.6: moment about the z-axis. 
LCID 
SF 
CID1 
Load  curve  ID    or  function  ID  .    The  applied  force  is  a  function  of  the
applicable degree-of-freedom of NODE2. 
Load curve scale factor. 
Coordinate system ID (optional), see remark 1 on next page. 
NODE2 
Node ID for calculating the force.
*LOAD_MOTION_NODE 
DESCRIPTION
DOF2 
Applicable degrees-of-freedom: 
EQ.1:  x-coordinate 
EQ.2:  y-coordinate, 
EQ.3:  z-coordinate, 
EQ.4:  x-translational displacement, 
EQ.5:  y-translational displacement, 
EQ.6:  z-translational displacement, 
EQ.7:  rotational displacement about the x-axis, 
EQ.8:  rotational displacement about the y-axis, 
EQ.9:  rotational displacement about the z-axis. 
EQ.10: x-translational velocity, 
EQ.11: y-translational velocity, 
EQ.12: z-translational velocity, 
EQ.13: rotational velocity about the x-axis, 
EQ.14: rotational velocity about the y-axis, 
EQ.15: rotational velocity about the z-axis. 
CID2 
Coordinate system ID (optional), see Remark 1. 
Remarks: 
1.  The  global  coordinate  system  is  the  default.    The  local  coordinate  system  ID’s 
are defined in the *DEFINE_COORDINATE_SYSTEM section.
*LOAD 
Purpose:    Apply  moving  pressure  loads  to  a  nondisjoint  surface.    The  pressure  loads 
approximate  a  jet  of  high  velocity  fluid  impinging  on  the  surface.    Multiple  surfaces 
may be defined each acted on by a set of nozzles. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LOADID 
Type 
I 
Default 
none 
Nozzle Cards.  Define the following cards for each nozzle.  Include as many cards as 
desired.  This input ends at the first card with the second field (NODE2) <= 3. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NODE1 
NODE2 
LCID 
CUTOFF 
LCIDT 
LCIDD 
Type 
I 
I 
I 
F 
Default 
none 
none 
none 
none 
I 
0 
I 
0 
The following card defines the surface where the nozzles act. 
  Card 3 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
IDTYPE 
NIP 
Type 
I 
I 
I 
Default 
none 
none 
3x3 
  VARIABLE   
DESCRIPTION
LOADID 
Loading ID. 
NODE1 
Node located at the origin of the nozzle.
*LOAD_MOVING_PRESSURE 
DESCRIPTION
NODE2 
Node located at the head of the nozzle 
LCID 
CUTOFF 
LCIDT 
LCIDD 
ID 
IDT 
Load  curve  or  function    ID  defining 
pressure versus radial distance from the center of the jet. 
Outer radius of jet.  The pressure acting outside this radius is set
to zero. 
Load  curve  or  function      ID,  which 
scales  the  pressure  as  a  function  of  time.    If  a  load  curve  isn’t
specified, the scale factor defaults to 1.0. 
Load  curve  or  function      ID,  which 
scales the pressure as a function of distance from the nozzle.  If a 
load curve isn’t specified, the scale factor defaults to 1.0. 
Segment set ID, shell element set ID, part set ID, or part ID.  See
IDT below. 
Slave segment or node set type.  The type must correlate with the
number specified for SSID: 
EQ.0: segment set ID for surface-to-surface contact, 
EQ.1: shell element set ID for surface-to-surface contact, 
EQ.2: part set ID, 
EQ.3: part ID, 
NIP 
Number  of  integration  in  segment  used  to  compute  pressure
loads.
Available options include: 
POINT 
SET 
*LOAD 
Purpose:  Apply a concentrated nodal force to a node or each node in a set of nodes. 
Node/Node  set  Cards.    Include  as  many  cards  as  necessary.    This  input  ends  at  the 
next keyword (“*”) card. 
Card 
1 
2 
3 
Variable  NID/NSID 
DOF 
LCID 
Type 
I 
I 
I 
4 
SF 
F 
Default 
none 
none 
none 
1. 
Remarks 
7 
M2 
I 
0 
8 
M3 
I 
0 
5 
CID 
I 
0 
1 
6 
M1 
I 
0 
2 
  VARIABLE   
DESCRIPTION
NID/NSID 
Node ID or nodal set ID (NSID), see *SET_NODE_OPTION. 
DOF 
Applicable degrees-of-freedom: 
EQ.1: 𝑥-direction of load action, 
EQ.2: 𝑦-direction of load action, 
EQ.3: 𝑧-direction of load action, 
EQ.4: follower force , 
EQ.5: moment about the 𝑥-axis , 
EQ.6: moment about the 𝑦-axis axis , 
EQ.7: moment about the 𝑧-axis axis , 
EQ.8: follower moment . 
LCID 
Load  curve  ID    or  function  ID  .
m1
m3m3
m2
Figure 27-3.  Nodes M1, M2, and M3 define a plane.  A positive follower force
acts in the positive 𝑡-direction of that plane, i.e., along the normal vector of the
plane.    A  positive follower  moment  puts a counterclockwise torque about the
normal  vector.    The  normal  vector  is  found  by  the  cross  product  𝐭 = 𝐯 × 𝐰
where 𝐯 and 𝐰 are vectors as shown. 
  VARIABLE   
DESCRIPTION
Load curve scale factor. 
Coordinate system ID (optional), see Remark 1 on next page. 
Node 1 ID.  Only necessary if DOF.EQ.4 or 8, see Remark 2 below.
Node 2 ID.  Only necessary if DOF.EQ.4 or 8, see Remark 2 below.
Node 3 ID.  Only necessary if DOF.EQ.4 or 8, see Remark 2 below.
SF 
CID 
M1 
M2 
M3 
Remarks: 
1.  Coordinate  Systems.    The  global  coordinate  system  is  the  default.    The  local 
coordinate  system  ID’s  are  defined  in  the  *DEFINE_COORDINATE_SYSTEM 
section. 
2.  Follower Forces.  The current position of nodes 𝑀1, 𝑀2, 𝑀3 are used to control 
the  direction  of  a  follower  force.    A  positive  follower  force  acts  normal  to  the 
plane defined by these nodes, and a positive follower moment puts a counter-
clockwise  torque  about  the  𝑡-axis.    These  actions  are  depicted  in  Figure  27-3.   
An  alternative  way  to  define  the  force  direction  is  by  setting  𝑀3  to  any  non-
positive value, in which case the follower force is in the  𝑀1 𝑡𝑜 𝑀2  direction. 
3.  Axisymmetric  Elements  with  Area  and  Volume  Weighting.    For  shell 
formulations 14 and 15, the axisymmetric solid elements with area and volume 
weighting, respectively, the specified nodal load is per unit length (type14) and 
per radian (type 15).
4.  Moments.  Moments can only be applied to nodes that have rotational degrees 
of  freedom.    Element  type  and  formulation  determine  the  degrees  of  freedom 
for  a  node,  e.g.,  the  nodes  of  solid  formulation  1  have  only  3  translational  de-
grees of freedom and no rotational degrees of freedom. 
5. 
*DEFINE_FUNCTION  for  LCID.    The  function  defined  by  LCID  has  7 
arguments: time, the 3 current coordinates, and the 3 reference coordinates.  A 
function that applies a force proportional to the distance from the initial coordi-
nates would be: 
f(t,x,y,z,x0,y0,z0)= -10.*sqrt ( (x-x0)*(x-x0)+(y-y0)*(y-y0)+(z-z0)*(z-z0) ) 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *LOAD_NODE_SET 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  A cantilever beam (made from shells) is loaded on the two end nodes 
$  (nodes 21 & 22).  The load is applied in the y-direction (dof=2). 
$  Load curve number 1 defines the load, but is scaled by sf=0.5 in the 
$  *LOAD_NODE_SET definition. 
$ 
*LOAD_NODE_SET 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$     nsid       dof      lcid        sf       cid        m1        m2        m3 
        14         2         1       0.5 
$ 
$ 
*SET_NODE_LIST 
$      sid 
        14 
$ 
$     nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
        21        22  
$ 
$ 
*DEFINE_CURVE 
$     lcid      sidr      scla      sclo      offa      offo 
         1 
$ 
$           abscissa            ordinate 
                 0.0                 0.0 
                10.0               100.0 
                20.0                 0.0 
$ 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
Available options include: 
<BLANK> 
SET 
*LOAD_REMOVE_PART 
Purpose:    Delete  the  elements  of  a  part  in  a  staged  construction  simulation.    Shock 
effects  are  prevented  by  gradually  reducing  the  stresses  prior  to  deletion.    Available 
only for solid and shell elements. 
Note:  This keyword card will be available starting in release 3 of version 971. 
Part Cards.  Include as many cards as necessary.  This input ends at the next keyword 
(“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID/PSID 
TIME0 
TIME1 
STGR 
Type 
I 
Default 
none 
F 
0 
F 
0 
I 
0 
  VARIABLE   
DESCRIPTION
PID 
Part ID (or Part Set ID for the_SET option) for deletion 
Time at which stress reduction starts 
Time at which stresses become zero and elements are deleted 
Construction stage at which part is removed (optional) 
TIME0 
TIME1 
STGR 
Remarks: 
There are 3 methods of defining the part removal time: 
1.  TIME0, TIME1 override all the other methods if non-zero 
2.  STGR refers to the stage at which the part is removed – the stages are defined in 
*DEFINE_CONSTRUCTION_STAGES.  This is equivalent to setting TIME0 and
TIME1  equal  to  the  start  and  end  of  the  ramp  time  at  the  beginning  of  stage 
STGR. 
3. 
*DEFINE_STAGED_CONSTRUCTION_PART can be used instead of *LOAD_-
REMOVE_PART  to  define  this  loading.    During  initialization,  a  STIFFEN_-
PART card will be created and the effect is the same as using the STGA, STGR 
method described above.
*LOAD_RIGID_BODY 
Purpose:  Apply a concentrated nodal force to a rigid body.  The force is applied at the 
center of mass or a moment is applied around a global axis.  As an option, local axes can 
be defined for force or moment directions. 
Rigid Body Cards.  Include as many Rigid Body Cards as necessary.  This input ends at 
the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
Variable 
PID 
DOF 
LCID 
Type 
I 
I 
I 
4 
SF 
F 
Default 
none 
none 
none 
1. 
Remark 
7 
M2 
I 
0 
8 
M3 
I 
0 
5 
CID 
I 
0 
1 
6 
M1 
I 
0 
2 
  VARIABLE   
DESCRIPTION
PID 
DOF 
Part ID of the rigid body, see *PART_OPTION. 
Applicable degrees-of-freedom: 
EQ.1: x-direction of load action, 
EQ.2: y-direction of load action, 
EQ.3: z-direction of load action, 
EQ.4: follower force, see Remark 2, 
EQ.5: moment about the x-axis, 
EQ.6: moment about the y-axis, 
EQ.7: moment about the z-axis. 
EQ.8: follower moment, see Remark 2. 
LCID 
Load  curve  ID    or  function  ID  . 
GT.0: force as a function of time, 
LT.0:  force as a function of the absolute value of the rigid body
displacement.  This option only applies to load curves.
VARIABLE   
DESCRIPTION
Load curve scale factor 
Coordinate system ID 
Node 1 ID.  Only necessary if DOF.EQ.4 or 8, see Remark 2. 
Node 2 ID.  Only necessary if DOF.EQ.4 or 8, see Remark 2. 
Node 3 ID.  Only necessary if DOF.EQ.4 or 8, see Remark 2. 
SF 
CID 
M1 
M2 
M3 
Remarks: 
1.  The  global  coordinate  system  is  the  default.    The  local  coordinate  system  ID’s 
are defined in the *DEFINE_COORDINATE_SYSTEM section.  This local axis is 
fixed in inertial space, i.e., it does not move with the rigid body. 
2.  Nodes  M1,  M2,  M3  must  be  defined  for  a  follower  force  or  moment.    The 
follower  force  acts  normal  to  the  plane  defined  by  these  nodes  as  depicted  in 
Figure  27-3.    The  positive  t-direction  is  found  by  the  cross  product  𝑡 = 𝑣 × 𝑤 
where v and w are vectors as shown.  The follower force is applied at the center 
of mass.  A positive follower moment puts a counterclockwise torque about the 
t-axis. 
3.  When  LCID  defines  a  function,  the  function  has  seven  arguments:  time,  the  3 
current  coordinates  for  the  center  of  mass,  and  the  3 reference  coordinates.    A 
function that applies a force proportional to the distance from the initial coordi-
nates would be  
f(t,x,y,z,x0,y0,z0)= -10.*sqrt ( (x-x0)*(x-x0)+(y-y0)*(y-y0)+(z-z0)*(z-z0) ).
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *LOAD_RIGID_BODY 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  From a sheet metal forming example.  A blank is hit by a punch, a binder is 
$  used to hold the blank on its sides.  The rigid holder (part 27) is held 
$  against the blank using a load applied to the cg of the holder. 
$ 
$  The direction of the load is in the y-direction (dof=2) but is scaled 
$  by sf = -1 so that the load is in the correct direction.  The load 
$  is defined by load curve 12. 
$ 
*LOAD_RIGID_BODY 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      pid       dof      lcid        sf       cid        m1        m2        m3 
        27         2        12      -1.0 
$ 
$ 
*DEFINE_CURVE 
$     lcid      sidr      scla      sclo      offa      offo 
        12 
$ 
$           abscissa            ordinate 
           0.000E+00           8.000E-05 
           1.000E+04           8.000E-05 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
*LOAD 
To define an ID for the segment loading, the following option is available: 
ID 
If the ID is defined an additional card is required. 
Purpose:    Apply  the  distributed  pressure  load  over  one  triangular  or  quadrilateral 
segment  defined  by  four,  six,  or  eight  nodes,  or  in  the  case  of  two-dimensional 
geometries,  over  one  two-noded  line  segment.    The  pressure  and  node  numbering 
convention follows the Figure 27-4 shown in the remarks below. 
ID Card.  Additional card for the ID keyword option. 
  Card 1 
Variable 
1 
ID 
Type 
I 
2 
3 
4 
5 
6 
7 
8 
HEADING 
A70 
  Card 2 
1 
Variable 
LCID 
Type 
I 
2 
SF 
F 
3 
AT 
F 
4 
N1 
I 
5 
N2 
I 
6 
N3 
I 
7 
N4 
I 
8 
N5 
I 
Default 
none 
1. 
0. 
none 
none 
none 
none 
none 
Remarks 
1 
2 
3 
4,5,6,7
n 3 
s  
n 
6 
n 
5 
n 1 
n 
4 
n 
2 
n 4 
n 
8 
n 1 
t 
n 
7 
n 
5 
n 3 
n 
6 
n 
Figure  27-4.    Nodal  numbering  for  pressure  segments  in  three-dimensional
geometries.  Positive pressure acts in the negative t-direction. 
4 
5 
6 
7 
8 
Addition card for when N5 ≠ 0. 
  Card 3 
Variable 
1 
N6 
Type 
I 
2 
N7 
I 
3 
N8 
I 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION
ID 
Loading ID 
HEADING 
A description of the loading. 
LCID 
Load  curve  ID    or  function  ID  . 
SF 
Load curve scale factor
VARIABLE   
DESCRIPTION
Arrival time for pressure or birth time of pressure. 
Node ID 
Node ID 
Node ID   
Node ID.  Repeat N3 for 3-node triangular segments. 
Mid-side node ID, if applicable . 
Mid-side node ID, if applicable . 
Mid-side node ID, if applicable . 
Mid-side node ID, if applicable . 
AT 
N1 
N2 
N3 
N4 
N5 
N6 
N7 
N8 
Remarks: 
1. 
If LCID is input as -1, then the Brode function is used to determine the pressure 
for the segments, see *LOAD_BRODE.  If LCID is input as -2, then an empirical 
airblast  function  is  used  to  determine  the  pressure  for  the  segments,  see 
*LOAD_BLAST. 
2.  The  load  curve  multipliers  may  be  used  to  increase  or  decrease  the  pressure.  
The time value is not scaled. 
3.  The activation time, AT, is the time during the solution that the pressure begins 
to act.  Until this time, the pressure is ignored.  The function value of the load 
curves  will  be  evaluated  at  the  offset  time  given  by  the  difference  of  the  solu-
tion time and AT i.e., (solution time-AT). 
4.  Triangular  segments  without  mid-side  nodes  are  defined  by  setting  N4 = N3.  
To apply a uniform pressure to type 17 tetrathedral elements, 4 triangular seg-
ments should be defined for each loaded face of an element.  Three of the seg-
ments should each have one corner node and the two adjacent mid-side node.  
The 4th segment should be made from the 3 mid-side nodes.   
5.  To  apply  a  uniform  pressure  to  type  16  tetrahedral  elements  or  type  24  type 
triangular shell elements, one 6 node segment may be defined for each loaded 
face.  However, LS-DYNA will accept and properly treat “any” other segment 
definition.    In  other  words,  if  the  preprocessor  happens  to  create  one  3-noded 
segment corresponding to local node numbering convention {1,2,3,3} in Figure
27-4, or permutations thereof, then this will internally be detected as a 6-noded 
segment  and  the  nodal  forces  will  be  consistently  distributed  over  the  6  in-
volved nodes.  Likewise, if four 3-noded segments corresponding to local node 
numbering  conventions  {1,4,6,6},  {2,5,4,4},    {3,6,5,5}  and  {4,5,6,6},  or  permuta-
tions  thereof,  are  created,  then  these  will  be  detected  to  belong  to  the  same  6-
noded segment and again result in the correct nodal forces. The difference be-
tween the two latter approaches is that using four “sub-segments” will provide 
four different normal directions 𝒕 instead of just one, and for curved faces this 
will provide a more accurate representation of the pressure load.  
6.  To  apply  a  uniform  pressure  to  type  23  hexahedral  elements  or  type  23 
quadrilateral shell elements, one 8 node segment may be defined for each load-
ed face.  However, LS-DYNA will accept and properly treat a segment exclud-
ing the 4 mid side nodes.  In other words, if the preprocessor happens to create 
just  one  4-noded  segment  corresponding  to  local  node  numbering  convention 
{1,2,3,4}  in  Figure  27-4,  or  permutations  thereof,  then  this  will  internally  be 
detected as a 8-noded segment and the nodal forces will be consistently distrib-
uted over the 8 involved nodes.  
7.  To apply a uniform pressure to type 24 hexahedral elements, either one 4 node 
segment corresponding to the numbering convention {1,2,3,4} in Figure 27-4, or 
permutations thereof, may be defined for each loaded face.  But LS-DYNA will 
also accept and properly treat four 4 node segments corresponding to {1,5,9,8}, 
{2,6,9,5}, {3,7,9,6} and {4,8,9,7}, where local node number 9 is located in the cen-
ter of the face. The difference between these two approaches is that using four 
“sub-segments”  will  provide  four  different  normal  directions  𝒕  instead  of  just 
one, and for curved faces this will provide a more accurate representation of the 
pressure load. 
8.  Segments  for  two-dimensional  geometries  are  defined  by  two  nodes,  N1  and 
N2.  Leave N3 and N4 as zero or else set both equal to N2.  A positive pressure 
acts  on  the  segment  in  the  Z  x  (N1-N2)  direction  where  Z  is  the  global  Z-axis 
and (N1-N2) is the vector from N1 to N2.   
9.  The function defined by LCID has 7 arguments: time, the 3 current coordinates, 
and the 3 reference coordinates.  A function that applies a pressure proportional 
to the distance from the initial coordinates would be: 
f(t,x,y,z,x0,y0,z0)= sqrt ( (x-x0)*(x-x0)+(y-y0)*(y-y0)+(z-z0)*(z-z0) )
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *LOAD_SEGMENT 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  A block of solid elements is pressed down onto a plane as it moves along 
$  that plane.  This pressure is defined using the *LOAD_SEGMENT keyword. 
$ 
$  The pressure is applied to the top of the block.  This top is defined 
$  by the faces on top of the appropriate solid elements.  The faces are 
$  defined with segments.  For example, nodes 97, 106, 107 & 98 define 
$  a top face on one of the solids (and thus, one of the faces to apply the 
$  pressure too).  This "face" is referred to as a single segment. 
$ 
$  The load is defined with load curve number 1.  The curve starts at zero, 
$  ramps to 100 in 0.01 time units and then remains constant.  However, 
$  the curve is then scaled by sclo = 2.5.  Thus, raising the load to 250. 
$  Note that the load is NOT scaled in the *LOAD_SEGMENT keyword, but 
$  could be using the sf variable. 
$ 
*LOAD_SEGMENT 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$     lcid        sf        at        n1        n2        n3        n4 
         1      1.00       0.0        97       106       107        98 
         1      1.00       0.0       106       115       116       107 
         1      1.00       0.0        98       107       108        99 
         1      1.00       0.0       107       116       117       108 
$ 
$ 
*DEFINE_CURVE 
$ 
$     lcid      sidr      scla      sclo      offa      offo 
         1         0       0.0       2.5 
$ 
$           abscissa            ordinate 
               0.000                 0.0 
               0.010               100.0 
               0.020               100.0 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
*LOAD_SEGMENT_CONTACT_MASK 
Purpose:    Mask  the  pressure  from  a  *LOAD_SEGMENT_SET  when  the  pressure 
segments  are  in  contact  with  another  material.    This  keyword  is  currently  only 
supported in the MPP version.  Note that the Heading Card is required. 
Heading Card. 
  Card 1 
Variable 
1 
ID 
Type 
I 
Load Set Card. 
  Card 2 
1 
Variable 
LSID 
Type 
I 
2 
3 
4 
5 
6 
7 
8 
HEADING 
A70 
2 
P1 
F 
3 
P2 
F 
4 
5 
6 
7 
8 
CID1 
CID2 
CID3 
CID4 
CID5 
I 
I 
I 
I 
I 
Optional Cards.  This data ends at the next “*” card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CID6 
CID7 
CID8 
CID9 
CID10 
CID11N 
CID12 
CID13 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
LSID 
P1 
Load  set  ID  to  mask,  which  must  match  a  *LOAD_SEGMENT_-
SET.  See Remark 2. 
Lower pressure limit.  When the surface pressure due to contact is
below  P1,  no  masking  is  done  and  the  full  load  defined  in
*LOAD_SEGMENT_SET  is  applied.    For  pressures  between  P1 
and P2 see Remark 1.
VARIABLE   
DESCRIPTION
P2 
CIDn 
Upper pressure limit.  When the surface pressure due to contact is
above P2, no load is applied due to the *LOAD_SEGMENT_SET. 
For pressures between P1 and P2 see Remark 1. 
The  IDs  of  contacts  that  can  mask  the  pressure  loads.    The
specified  contact  definitions  must  all  be  of  the  same  type.
Furthermore, only non-automatic SURFACE_TO_SURFACE (two 
way) or AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK are 
supported. 
For  TIEBREAK  contacts,  pressure  is  masked  until  the  tie  fails.
Once  the  tie  fails,  the  full  pressure  will  be  applied  for  the
remainder of the simulation.  The values P1 and P2 are ignored. 
For  other  contact  types,  the  contact  forces,  along  with  the  nodal
contact surface areas, are used to compute the contact pressure at
each node to determine any masking effect. 
Remarks: 
1. 
Intermediate Pressures.  If the contact pressure, 𝑝contact is between P1 and P2, 
the pressure load is scaled by a factor of 
P1 may be set equal to P2 if desired. 
𝑓 =
P2 − 𝑝contact
𝑃2 − 𝑃1
. 
2.  LSID.    The  LSID  values  must  be  unique.    Having  two  instances  of  this 
referencing  the  same*LOAD_SEGMENT_SET  is  not  supported.    However,  a 
contact ID may appear in two different instances of this keyword.
*LOAD_SEGMENT_FILE 
Purpose:    To  define  time-varying  distributed  pressure  loads  over  triangular  or 
quadrilateral segments defined by four, six, or eight nodes via a binary file. 
  Card 1 
Variable 
Type 
1 
FILENAME 
A80 
Card 2 is required but may be left blank. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
Type 
I 
Default 
none 
  VARIABLE   
FILENAME 
DESCRIPTION
Filename of binary database containing segment pressures versus
time.  There are three sections in this database. 
LCID 
Optional  Load  curve  ID  defining  segment  pressure  scale  factor 
versus time.
*LOAD_SEGMENT_FILE 
Each  database  is  assumed  to  be  written  with  a  block  size  equal  to  a  multiple  of  512 
words, with each block containing 1 or more states.  If the data does not complete the 
last  block  it  is  padded  with  zeros.    The  code  will  open  and  read  next  family  file  if  it 
detects phony word or EOF.  If the IO returns a zero length read, the code assumes end 
of IO and strop reading. 
Linear interpolation is used if IO can find current time between two states.  Therefore, 
the given database can have more states than simulation time steps. 
Linear  extrapolation will  only  be  used  when  IO  reaches  end  of  the  database.    The  last 
two  states  will  be  used  and  code  will  issue  warning  message  “MSG_SOL+1323”  to 
d3hsp and messag files. 
Section 
Words 
Description 
Control Section 
64 words 
Segment Data 
4 words 
Mid-side Nodes 4 
Words.  Ommitted 
unless NSEG < 0. 
10 
1 
1 
1 
1 
1 
1 
1 
1 
1 
Title 
NSEG:  The  absolute  value,  |"NSEG"  |  specifies  the 
number  of  segments  contained  within  the 
file.    If  NSEG < 0,  then  the  file  contains  mid-
side nodes. 
N1; Node ID. 
N2: Node ID. 
N3: Node  ID. 
geometries. 
  Repeat  N2  for  two-dimensional 
N4: Node  ID. 
  Repeat  N2  for  two-dimensional 
geometries  or  repeat  N3  for  3-node  triangular 
segments. 
N5: Optional mid-side node ID. 
N6: Optional mid-side node ID. 
N7: Optional mid-side node ID. 
N8: Optional mid-side node ID. 
⋮ 
4 or 8 
⋮ 
NSEGth segment data 
4 or 8 
Last set of segment data 
“State” Section 
1 + |NSEG| words 
1 
1 
⋮ 
Time 
Segment Pressure 
⋮
⋮ 
1 
1 
NSEG 
Pressure of last segment 
⋮ 
⋮
*LOAD 
Purpose:  Apply distributed pressure loads from a previous ALE analysis to a specified 
segment set in the current analysis.  This capability trades some of the model’s accuracy 
for a large reduction in model size. 
NOTE:  The  deck  for  the  “previous”  run  must  include  a 
*DATABASE_BINARY_FSILNK  card  to  activate  the 
creation  of  the  fsilink  file.    Either  the  *LOAD_SEG-
MENT_FSILNK  card  (this  card)  or  the  *DATA-
BASE_BINARY_FSILNK  card  may  be  in  an  input 
deck, but not both. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
FILENAME 
A80 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NINT 
LCID 
Type 
I 
Default 
none 
I 
0 
Coupling  ID  Cards.    Read  in  NINT  coupling  IDs.    Repeat  this  card  as  many  times  as 
necessary to input all NINT values. 
  Card 3 
1 
Variable 
ID1 
2 
ID2 
3 
ID3 
4 
ID4 
5 
ID5 
6 
ID6 
7 
ID7 
8 
ID8 
Type 
I 
I 
Default 
none 
none
*LOAD_SEGMENT_FSILNK 
DESCRIPTION
FILENAME 
Filename of the interface linking file. 
NINT 
LCID 
IDi 
Number  of  couplings  for  which  the  previous  run  provides
pressure data. 
Load  curve  ID    or  function  ID  .    The  curve  referred  to  by  LCID  provides  a
scale factor as a function of time.  The pressure data that is read in
from the fsilnk file is scaled according to this value. 
These  must  match  COUPIDs  from  the  *CONSTRAINED_LA-
GRANGE_IN_SOLID  card  from  the  previous  runs.    These  IDs
specify which of the first run’s couplings are propagated into this
run through pressure data read from the fsilnk file. 
The algorithm: 
This  feature  provides  a  method  for  using  pressure  time  history  data  from  *CON-
STRAINED_LAGRANGE_IN_SOLID  Lagrangian-to-ALE  couplings  in  one  calculation 
as  pressure  data  for  the  same  segment  in  subsequent  calculations.    The  time  range 
covered  by  the  subsequent  calculation  must  overlap  the  time  range  of  the  initial 
calculation. 
First calculation: Write out pressure data. 
1.  Add a *DATABASE_BINARY_FSILNK card to the first run. 
2.  Specify  filename  for  the  fsilnk  file  by  adding  a  command  line  argument  to  ls-
dyna. 
ls-dyna … fsilnk=fsi_filename … 
Without  a  *DATABASE_BINARY_FSILNK  card  this  command  line  argument 
will have no effect. 
Format of fsilnk File: 
WRITE: Job title (character*80 TITLE) 
WRITE: Number of interfaces (integer NINTF) 
For 𝑖 = 1 to NINTF { 
WRITE: Number of segments in the ith interface (integer NSEG[𝑖]) 
For 𝑗 = 1 to NSEG[𝑖] {
WRITE: Connectivities of jth segment in the ith interface (integer*4) 
} 
} 
For 𝑛 = 1 to number of time steps { 
WRITE: time value for the nth time step (real) 
For 𝑖 = 1 to NINTF 
For 𝑗 = 1 to NSEG[𝑖] { 
WRITE: Pressure for the jth segment of the ith interface (real) 
} 
} 
} 
Subsequent calculations: Read fsilnk File. 
Include  this  keyword,  *LOAD_SEGMENT_FSILNK,  and  be  careful  to  remove  the 
*DATABASE_BINARY_FSILNK  keyword.   Specify  the  name  of  the fsilnk  file  from  the 
previous run on *LOAD_SEGMENT_FSILNK’s first data card. 
Then,  at  each  time  step,  the  pressure  of  the  specified  coupling  IDs  is  set  on  the 
Lagrangian-mesh  side  from  data  in  the fsilnk  file.    For  times  outside  of  the fsilnk  file’s 
range LS-DYNA extrapolates. 
1. 
If current time is before the 1st fsilnk time, then pressure is set to 0. 
2. 
If the current time is in the range of times in the fsilnk file, then the pressure is 
linearly interpolated from the data at the two time states in the fsilnk file brack-
eting the current time. 
3. 
If  the  current  time  is  after  the  last  fsilnk  time,  then  the  pressure  is  set  to  the 
fsilnk pressure at last time step.
*LOAD_SEGMENT_NONUNIFORM_{OPTION} 
To define an ID for the non-uniform segment loading the following option is available: 
ID 
If the ID is defined an additional card is required. 
Purpose:  Apply a distributed load over one triangular or quadrilateral segment defined 
by three, four, six, or eight nodes.  The loading and node numbering convention follows 
Figure 27-3. 
ID Card.  Additional card for ID keyword option. 
 Optional 
Variable 
1 
ID 
Type 
I 
2 
3 
4 
5 
6 
7 
8 
HEADING 
A70 
Card  Sets.    Each  segment  is  specified  by  a  set  of  the  following  3  cards.    Include  as 
many sets as necessary.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
Variable 
LCID 
Type 
I 
2 
SF 
F 
3 
AT 
F 
4 
DT 
F 
Default 
none 
1. 
0. 
1.E+16
Remarks 
1 
2 
3 
3 
5 
CID 
I 
0 
4 
6 
V1 
F 
7 
V2 
F 
8 
V3 
F 
none 
none 
none
Card 2 
Variable 
1 
N1 
Type 
I 
2 
N2 
I 
3 
N3 
I 
4 
N4 
I 
5 
N5 
I 
6 
N6 
I 
7 
N7 
I 
8 
N8 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 3 
Variable 
1 
P1 
Type 
F 
2 
P2 
F 
3 
P3 
F 
4 
P4 
F 
5 
P5 
F 
6 
P6 
F 
7 
P7 
F 
8 
P8 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
ID 
Loading ID 
HEADING 
A description of the loading. 
LCID 
Load  curve  ID    or  function  ID  .    For  a  load  curve  ID  the  load  curve  must
provide  pressure  as  a  function  of  time.    For  a  function  ID,  the
function is expected to have seven arguments: current time minus
the birth time, the current x, y, and z coordinates, and the initial x,
y, and z coordinates. 
LT.0:  Applies to 3, 4, 6 and 8-noded segments.  With this option 
the load becomes a follower load, meaning that the direc-
tion  of  the  load  is  constant  with  respect  to  the  local  seg-
ment coordinate system. 
SF 
AT 
DT 
Load curve scale factor 
Arrival/birth time for the traction load. 
Death time for the traction load. 
CID 
Coordinate system ID
V1, V2, V3 
*LOAD_SEGMENT_NONUNIFORM 
DESCRIPTION
Vector  direction  cosines    relative  to  coordinate  system  CID
defining  the  direction  of  the  traction  loading.    Note  that  for
LCID.LT.0 this vector rotates with the geometry of the segment.  
N1 
N2 
N3 
N4 
N5 
N6 
N7 
N8 
P1 
P2 
P3 
P4 
P5 
P6 
P7 
P8 
Node ID 
Node ID 
Node ID.  Repeat N2 for two-dimensional geometries. 
Node ID.  Repeat N2 for two-dimensional geometries or repeat N3
for 3-node triangular segments. 
Optional mid-side node ID . 
Optional mid-side node ID .   
Optional mid-side node ID . 
Optional mid-side node ID . 
Scale factor at node ID, N1. 
Scale factor at node ID, N2. 
Scale factor at node ID, N3. 
Scale factor at node ID, N4. 
Scale factor at node ID, N5. 
Scale factor at node ID, N6. 
Scale factor at node ID, N7. 
Scale factor at node ID, N8.
*LOAD 
To define an ID for the segment loading, the following option is available: 
ID 
If the ID is defined an additional card is required. 
Purpose:  Apply the distributed pressure load over each segment in a segment set.  See 
*LOAD_SEGMENT  for  a  description  of  the  pressure  sign  convention  and  remarks  on 
high order segment definitions. 
ID Card.  Additional card for the ID keyword option.  
 Optional 
Variable 
1 
ID 
Type 
I 
2 
3 
4 
5 
6 
7 
8 
HEADING 
A70 
Segment Set Cards.  Include as many segment set cards as necessary.  This input ends 
at the next keyword (“*”) card. 
5 
6 
7 
8 
  Card 1 
1 
2 
Variable 
SSID 
LCID 
Type 
I 
I 
3 
SF 
F 
Default 
none 
none 
1. 
Remarks 
1 
2 
4 
AT 
F 
0. 
3 
  VARIABLE   
DESCRIPTION
SSID 
Segment set ID, see *SET_SEGMENT.
Load  curve  ID    or  function  ID  .    For  a  load  curve  ID  the  load  curve  must
provide  pressure  as  a  function  of  time.    For  a  function  ID  the
function is expected to have seven arguments: current time minus
the birth time, the current x, y, and z coordinates, and the initial x, 
y, and z coordinates. 
Load curve scale factor 
Arrival time for pressure or birth time of pressure. 
*LOAD 
  VARIABLE   
LCID 
SF 
AT 
Remarks: 
1. 
If LCID is input as -1, then the Brode function is used to determine pressure for 
the segment set, also see *LOAD_BRODE.  If LCID is input as -2, then an empir-
ical  airblast    function  is  used  to  determine  the  pressure  for  the  segments,  see 
*LOAD_BLAST. 
2.  The  load  curve  multipliers  may  be  used  to  increase  or  decrease  the  pressure.  
The time value is not scaled. 
3.  The activation time, AT, is the time during the solution that the pressure begins 
to act.  Until this time, the pressure is ignored.  The function value of the load 
curves  will  be  evaluated  at  the  offset  time  given  by  the  difference  of  the  solu-
tion time and AT i.e., (solution time-AT).
*LOAD 
Purpose:    Apply  the  traction  load  over  a  segment  set  that  is  dependent  on  the 
orientation of a vector.  An example application is applying a pressure to a cylinder as a 
function of the crank angle in an automobile engine.  The pressure and node numbering 
convention follows Figure 27-4. 
Card Sets.  Include as many  sets of Cards  1 and 2 as desired.  This input ends at the 
next keyword (“*”) card. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
IDSS 
LCID 
SCALE 
IOPTP 
IOPTD 
I 
0 
5 
I 
0 
6 
7 
8 
Type 
I 
I 
I 
F 
Default 
none 
none 
none 
1. 
  Card 2 
Variable 
1 
N1 
Type 
I 
2 
N2 
I 
3 
NA 
I 
4 
NI 
I 
Default 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
ID 
IDSS 
LCID 
Loading ID 
Segment set ID. 
Load  curve  or  function  ID  defining  the  traction  as  a  function  of
the  angle.    If  IOPT = 0  below,  define  the  abscissa  between  0  and 
2π radians or 0 and 360 degrees if IOPD = 1. 
SCALE 
Scale factor on value of the load curve or function.
IOPTP 
*LOAD_SEGMENT_SET_ANGLE 
DESCRIPTION
Flag  for  periodicity.    The  default  (IOPTP = 0)  requires  the  load 
curve to be defined between 0 and 2π.  This is useful, for example, 
for modeling an engine that is running at a steady state since each 
rotation  will  experience  the  same  loading.    To  model  a  transient
response, IOPTP = 1 uses a load curve defined over the full range
of  angles,  permitting  a  different  response  on  the  second  and
subsequent revolutions. 
IOPTD 
Flag  for  specifying  if  the  load  curve  or  function  argument  is  in
radians (IOPTD = 0, the default) or degrees (IOPTD = 1). 
N1 
N2 
NA 
NI 
The node specifying the tail of the rotating vector. 
The node specifying the head of the rotating vector. 
The  node  specifying  the  head  of  the  vector  defining  the  axis  of
rotation.  The node N1 specifies the tail. 
The  node  specifying  the  orientation  of  the  vector  at  an  angle  of
zero.  If the initial angle is zero, NI should be equal to N2. 
z 
y 
x 
N2 
initial 
α, 
angle 
N1 
NI 
NA
*LOAD_SEGMENT_SET_NONUNIFORM_{OPTION} 
To define an ID for the non-uniform segment loading the following option is available: 
ID 
If the ID is defined an additional card is required. 
Purpose:  Apply the traction load over one triangular or quadrilateral segment defined 
by  three or  four  nodes.    The  pressure  and  node  numbering  convention  follows Figure 
27-4. 
ID Card.  Additional card for ID keyword option.  
 Optional 
Variable 
1 
ID 
Type 
I 
2 
3 
4 
5 
6 
7 
8 
HEADING 
A70 
Card Sets.  Include as many pairs of Cards 1 and 2 as desired.  This input ends at the 
next keyword (“*”) card. 
  Card 1 
1 
2 
Variable 
SSID 
LCID 
Type 
I 
I 
3 
SF 
F 
Default 
none 
none 
1. 
  Card 2 
1 
Variable 
CID 
Type 
Default 
I 
0 
2 
V1 
F 
3 
V2 
F 
none 
none 
none 
5 
6 
7 
8 
DT 
ELTYPE 
F 
A 
1016 
none 
5 
6 
7 
8 
4 
AT 
F 
0. 
4 
V3
N4
Edge 4
N1
Edge 1
Edge 3
N3
Edge 2
N2
Figure 27-5.  Local coordinates system for edge load. 
  VARIABLE   
DESCRIPTION
ID 
Loading ID 
HEADING 
A description of the loading. 
SSID 
LCID 
Segment set ID. 
Load  curve  ID    or  function  ID  .    The  seven  arguments  for  the  function  are 
current  time  minus  the  birth  time,  the  current  x,  y,  and  z
coordinates, and the initial x, y, and z coordinates. 
LT.0:  Applies  to  3,  4,  6  and  8-noded  segment  sets.    With  this 
option  the  load  becomes  a  follower  load,  meaning  that
the  direction  of  the  load  is  constant  with  respect  to  the
local  segment  coordinate  system.    The  local  coordinate
system  for  edge  load,  see  ELTYPE,  is  shown  in  Fig-
ure 27-5. 
SF 
AT 
DT 
Load curve scale factor 
Arrival/birth time for pressure. 
Death time for pressure.
VARIABLE   
ELTYPE 
DESCRIPTION
Optional  edge  loading  type.    If  left  blank,  pressure  on  the
segment will be applied. 
EQ.EF1: Distributed  force  per  unit  length  along  edge  1,
Figure 27-5. 
EQ.EF2: Distributed  force  per  unit  length  along  edge  2,
Figure 27-5. 
EQ.EF3: Distributed  force  per  unit  length  along  edge  3, 
Figure 27-5. 
EQ.EF4: Distributed  force  per  unit  length  along  edge  4,
Figure 27-5. 
CID  
Coordinate system ID 
V1, V2, V3 
Vector  direction  cosines  relative  to  the  coordinate  system  CID
defining  the  direction  of  the  traction  loading.    Note  that  for
LCID.LT.0 this vector rotates with the geometry of the segment.
*LOAD_SEISMIC_SSI_OPTION1_{OPTION2} 
Available options for OPTION1 include: 
NODE 
SET 
POINT 
OPTION2 allows an optional ID to be given: 
ID 
Purpose:  Apply earthquake load due to free-field earthquake ground motion at certain 
locations — defined by either nodes or coordinates — on a soil-structure interface, for 
use in earthquake soil-structure interaction analysis.  The specified motions are used to 
compute  a  set  of  effective  forces  in  the  soil  elements  adjacent  to  the  soil-structure 
interface, according to the effective seismic input–domain reduction method [Bielak and 
Christiano (1984)].  
ID Card.  Additional card for the ID keyword option. 
 Optional 
Variable 
1 
ID 
Type 
I 
2 
3 
4 
5 
6 
7 
8 
HEADING 
A70 
Card Sets.  Include as many pairs of Cards 1 and 2 as desired.  This input ends at the 
next keyword (“*”) card. 
Node and set Cards.  Card 1 for keyword options NODE or SET: 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
typeID 
GMX 
GMY 
GMZ 
Type 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none
Point Cards.  Card 1 for keyword option POINT. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
SSID 
Type 
I 
Default 
none 
XP 
F 
0. 
YP 
F 
0. 
ZP 
F 
0. 
GMX 
GMY 
GMZ 
I 
I 
I 
none  none  none 
  Card 2 
Variable 
1 
SF 
2 
3 
4 
5 
6 
7 
8 
CID 
BIRTH 
DEATH 
ISG 
IGM 
Type 
F 
Default 
1. 
I 
0 
F 
0. 
F 
1028 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
ID 
Optional ID.  This ID does not need to be unique. 
HEADING 
An optional descriptor for the given ID. 
SSID 
Soil-structure interface ID. 
typeID 
Node ID (NID in *NODE) or nodal set ID (SID in *SET_NODE). 
XP 
YP 
ZP 
GMX 
GMY 
GMZ 
𝑥 coordinate of ground motion location on soil-structure interface.
𝑦 coordinate of ground motion location on soil-structure interface.
𝑧 coordinate of ground motion location on soil-structure interface.
Acceleration  load  curve  or  ground  motion  ID  for  motion  in  the
(local) 𝑥-direction. 
Acceleration  load  curve  or  ground  motion  ID  for  motion  in  the
(local) 𝑦-direction. 
Acceleration  load  curve  or  ground  motion  ID  for  motion  in  the
(local) 𝑧-direction.
SF 
CID 
*LOAD_SEISMIC_SSI 
DESCRIPTION
Ground motion scale factor.  (default = 1.0) 
Coordinate system ID, see *DEFINE_COORDINATE_SYSTEM. 
BIRTH 
Time at which specified ground motion is activated. 
DEATH 
Time at which specified ground motion is removed: 
EQ.0.0: default set to 1028 
ISG 
Definition of soil-structure interface: 
EQ.0: SSID is ID for soil-structure interface defined by *INTER-
FACE_SSI_ID  for  non-matching  mesh  between  soil  and 
structure. 
EQ.1: SSID is segment set ID identifying soil-structure interface 
for merged meshes between soil and structure. 
IGM 
Specification of ground motions GMX, GMY, GMZ: 
EQ.0: ground motions are specified as acceleration load curves.
See *DEFINE_CURVE 
EQ.1: Both  ground  accelerations  and  velocities  specified  using
*DEFINE_GROUND_MOTION. 
Remarks: 
1.  The  ground  motion  at  any  node  on  a  soil-structure  interface  is  computed  as 
follows:   
a)  If  the  node  coincides  with  a  location  where  ground  motion  is  specified, 
that ground motion is used for that node. 
b)  If  the  node  does  not  coincide  with  a  location  where  ground  motion  is 
specified,  the  ground  motion  at  that  node  along  a  particular  degree-of-
freedom  is  taken  as  a  weighted  average  of  all  the  ground  motions  speci-
fied on the interface along that degree-of-freedom, where the weights are 
inversely proportional to the distance of the node from the ground motion 
location. 
2.  Multiple  ground  motions  specified  at  the  same  location  are  added  together  to 
obtain the resultant ground motion at that location.
3.  Spatially-uniform ground motion may be specified on a soil-structure interface 
by specifying the ground motion at only one location on that interface.  Specify-
ing  the ground  motion  at  more  than one  point  on  a  soil-structure interface  re-
sults in spatially-varying ground motion on that interface.
*LOAD_SHELL_OPTION1_{OPTION2} 
Available options for OPTION1 include: 
ELEMENT 
SET 
Available options for OPTION2 include: 
ID 
If the ID is defined an additional card is required. 
Purpose:    Apply  the  distributed  pressure  load  over  one  shell  element  or  shell  element 
set.    The  numbering  of  the  shell  nodal  connectivities  must  follow  the  right  hand  rule 
with positive pressure acting in the negative t-direction.  See Figure 27-4.  This option 
applies to the three-dimensional shell elements only. 
ID Card.  Additional card for ID keyword option. 
 Optional 
Variable 
1 
ID 
Type 
I 
2 
3 
4 
5 
6 
7 
8 
HEADING 
A70 
Shell  Cards.    Include  as  many  of  these  cards  as  desired.    This  input  ends  at  the  next 
keyword (“*”) card. 
5 
6 
7 
8 
  Card 1 
1 
2 
Variable 
EID/ESID 
LCID 
Type 
I 
I 
3 
SF 
F 
Default 
none 
none 
1. 
Remarks 
1 
1 
2 
4 
AT 
F 
0.
EID/ESID 
*LOAD 
DESCRIPTION
Shell  ID  (EID)  or  shell  set  ID  (ESID),  see  *ELEMENT_SHELL  or 
*SET_SHELL. 
LCID 
Load curve ID, see *DEFINE_CURVE. 
Load curve scale factor 
Arrival time for pressure or birth time of pressure. 
SF 
AT 
Remarks: 
1. 
2. 
If LCID is input as -1, then the Brode function is used to determine the pressure 
for the segments, see also *LOAD_BRODE. 
If  LCID  is  input  as  -2,  then  the  ConWep  function  is  used  to  determine  the 
pressure for the segments, see *LOAD_BLAST. 
3.  The  load  curve  multipliers  may  be  used  to  increase  or  decrease  the  pressure.  
The time value is not scaled. 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *LOAD_SHELL_ELEMENT 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  From a sheet metal forming example.  A blank is hit by a punch, a holder is 
$  used to hold the blank on its sides.  All shells on the holder are given a 
$  pressure boundary condition to clamp down on the blank.  The pressure 
$  follows load curve 3, but is scaled by -1 so that it applies the load in the 
$  correct direction.  The load starts at zero, but quickly rises to 5 MPa 
$  after 0.001 sec.  (Units of this model are in: ton, mm, s, N, MPa, N-mm) 
$ 
*LOAD_SHELL_ELEMENT 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      eid      lcid        sf        at 
     30001         3 -1.00E+00       0.0 
     30002         3 -1.00E+00       0.0 
     30003         3 -1.00E+00       0.0 
     30004         3 -1.00E+00       0.0 
     30005         3 -1.00E+00       0.0 
     30006         3 -1.00E+00       0.0 
     30007         3 -1.00E+00       0.0 
$ 
$  Note: Just a subset of all the shell elements of the holder is shown above, 
$        in practice this list contained 448 shell element id's. 
$ 
$ 
*DEFINE_CURVE 
$     lcid      sidr      scla      sclo      offa      offo 
         3 
$
$           abscissa            ordinate 
               0.000                 0.0 
               0.001                 5.0 
               0.150                 5.0 
$ 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
*LOAD 
Purpose:  When used in a full-deck restart run, this card will apply the SPC constraint 
forces from the initial run on the corresponding degrees of freedom in the current run.  
This  is  useful  when  modeling  unbounded  domains  using  a  non-reflecting  boundary 
while incorporating static stresses computed in the initial run: the fixed constraints on 
the  outer  boundary  in  the  initial  static  analysis  are  removed  in  the  transient  analysis 
and replaced by equivalent static forces.  
While  *BOUNDARY_NON_REFLECTING  acts  similarly  if  dynamic  relaxation  is  used 
for the static analysis, this approach works for any method used to preload the model. 
No parameters are necessary for this card.
*LOAD_SSA 
Purpose:    The  Sub-Sea  Analysis  (SSA)  capability  allows  a  simple  and  efficient  way  of 
loading  the  structure  to  account  for  the  effects  of  the  primary  shock  wave  and  the 
subsequent bubble oscillations of an underwater explosion.  It achieves its efficiency by 
approximating the pressure scattered by air and water-backed plates and the pressure 
transmitted  through  a  water-back  plate.    The  loading  incorporates  the  plane  wave 
approximation for direct shock response and the virtual mass approximation for bubble 
response.    *LOAD_SSA  does  not  implement  a  doubly  asymptotic  approximation  of 
transient fluid-structure interaction. 
  Card 1 
Variable 
1 
VS 
Type 
F 
2 
DS 
F 
3 
REFL 
F 
Default 
none 
none 
0. 
4 
ZB 
F 
0. 
5 
6 
7 
8 
ZSURF 
FPSID 
PSID 
NPTS 
F 
0. 
I 
0 
I 
0 
I 
1 
Card Sets.  Include as many pairs of Cards 1 and 2 as necessary.  This input ends at the 
next keyword (“*”) card. 
  Card 1 
Variable 
Type 
1 
A 
F 
2 
3 
4 
5 
6 
7 
8 
ALPHA 
GAMMA 
KTHETA 
KAPPA 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
  Card 2 
Variable 
1 
XS 
Type 
F 
2 
YS 
F 
3 
ZS 
F 
4 
W 
F 
5 
6 
TDELY 
RAD 
F 
F 
7 
CZ 
F 
8 
Default 
none 
none 
none 
none 
none 
none 
none
VARIABLE   
DESCRIPTION
VS 
DS 
Sound speed in fluid 
Density of fluid 
REFL 
Consider reflections from sea floor. 
EQ.0: off 
EQ.1: on 
ZB 
Z coordinate of sea floor if REFL = 1, otherwise, not used. 
ZSURF 
Z coordinate of sea surface 
FPSID 
Part set ID of parts subject to flood control.  Use the *PART_SET_-
COLUMN  option  where  the  parameters  A1  and  A2  must  be
defined as follows: 
Parameter A1: Flooding status: 
EQ.1.0: Fluid on both sides. 
EQ.2.0: Fluid outside, air inside. 
EQ.3.0: Air outside, fluid inside. 
EQ.4.0: Material or part is ignored. 
Parameter A2: Tubular outer diameter of beam elements.  For
shell elements this input must be greater than zero for loading.
PSID 
Part  set  IDs  of  parts  defining  the  wet  surface.    The  elements
defining  these  parts  must  have  their  outward  normals  pointing
into the fluid.  See Figure 27-6. 
EQ.0: all parts are included. 
GT.0: the part set id. 
NPTS 
Number of integration points for computing pressure (1 or 4) 
A 
Shock pressure parameter 
ALPHA 
α, shock pressure parameter 
GAMMA 
γ, time constant parameter
Elements covering the
surface must have outward
facing normal vectors
Figure 27-6.  The shell elements interacting with the fluid must be numbered
such that their outward normal vector points into the fluid media. 
  VARIABLE   
DESCRIPTION
KTHETA 
KAPPA 
𝐾𝜃, time constant parameter 
κ, ratio of specific heat capacities 
XS 
YS 
ZS 
W 
X coordinate of charge 
Y coordinate of charge 
Z coordinate of charge 
Weight of charge 
TDELY 
Time delay before charge detonates 
RAD 
CZ 
Charge radius 
Charge depth 
Remarks: 
1. 
 SSA  assumes  the  model  is  in  MKS  units.    If  it  is  in  another  system  of  units, 
*control_coupling should be used to account for the conversion.
2.  The  “flooding  status”  is instrumental  in  determining  how  the  model  parts  are 
loaded.    If  A1 = 1,  the  front  of  the  plate  as  defined  by  the  outward  normal  is 
exposed  to  the  incident  pressure.    The  back  of  the  plate  is  not  exposed  to  the 
incident  pressure  but  feels  a  transmitted  pressure  that  resists  plate  motion.    If 
A1 = 2, then the plating has fluid on the outside as determined by the outward 
normal.  It is exposed to the incident pressure and feels the scattered pressure.  
No loading is applied to the back side.  If A1 = 3, then air is on the front of the 
plate  and  water  is  on  the  back.    Neither  the  front  nor  the  back  of  the  plate  is 
exposed to the incident pressure, but the motion of the plate is resisted by pres-
sure generated on the back of the plate when it moves.  Transmitted pressures 
are assumed not to strike another plate. 
3.  The  pressure  history  of  the  primary  shockwave  at  a  point  in  space  through 
which a detonation wave passes is given as:  
𝑃(𝑡) = 𝑃𝑚𝑒
−𝑡
𝜃  
where 𝑃𝑚 and the time constant 𝜃 below are functions of the type and weight W 
of the explosive charge and the distance 𝑄 from the charge. 
𝑃𝑝𝑒𝑎𝑘 = 𝐴 [
]
𝑊1/3
𝜃 = 𝐾𝜃𝑊1/3 [
]
𝑊1/3
where A, α, γ, and Κθ are constants for the explosive being used.
*LOAD_STEADY_STATE_ROLLING 
Steady state rolling analysis is a generalization of *LOAD_BODY, allowing the user to 
apply  body  loads  to  part  sets  due  to  translational  and  rotational  accelerations  in  a 
manner  that  is  more  general  than  the  *LOAD_BODY  capability.    *LOAD_STEADY_-
STATE_ROLLING may be invoked multiple times as long as no part has the command 
applied  more  than  once.      Furthermore,  the  command  may  be  applied  to  arbitrary 
meshes, i.e., axisymmetric meshes are not required. 
Card Sets.  Include as many sets consisting of the following four cards as desired.  This 
input ends at the next keyword (“*”) card. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
PSID 
Type 
I 
I 
Default 
none 
none 
  Card 2 
Variable 
Type 
Default 
  Card 3 
Variable 
Type 4 
Default 
1 
N1 
I 
0 
1 
N3 
I 
0 
2 
N2 
I 
0 
2 
N4 
I 
0 
3 
4 
5 
6 
7 
8 
LCD1 
LCD1R 
I 
0 
3 
I 
0 
4 
LCD2 
LCD2R 
I 
0 
I 
0 
5 
6 
7
Card 4 
Variable 
Type 
Default 
1 
N5 
I 
0 
2 
N6 
I 
0 
3 
4 
5 
6 
7 
8 
LCD3 
LCD3R 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
ID 
PSID 
N1 
N2 
ID 
Part set ID 
Node 1 defining rotational axis 
Node 2 defining rotational axis 
LCD1 
Load curve defining angular velocity around rotational axis. 
LCD1R 
Optional  load  curve  defining  angular  velocity  around  rotational
axis  for  dynamic  relaxation.    LCD1  is  used  during  dynamic
relaxation if LCD1R is not defined. 
N3 
N4 
Node 3 defining turning axis 
Node 4 defining turning axis 
LCD2 
Load curve defining angular velocity around turning axis. 
LCD2R 
N5 
N6 
LCD3 
LCD3R 
Optional  load  curve  defining  angular  velocity  around  turning
axis  for  dynamic  relaxation.    LCD2  is  used  during  dynamic
relaxation if LCD2R is not defined. 
Node 5 defining translational direction 
Node 6 defining translational direction 
Load  curve  defining  translational  velocity 
direction. 
in  translational
load 
in
Optional 
translational direction.  LCD3 is used during dynamic relaxation
if LCD3R is not defined. 
translational  velocity 
curve  defining
*LOAD_STEADY_STATE_ROLLING 
The  steady  state  rolling  capability  adds  inertial  body  loads  in  terms  of  a  moving 
reference defined by the user input.  The current coordinates are defined in terms of the 
displacement, u, and the moving reference frame, Y, 
𝑥𝑆𝑆𝑅 = 𝑢 + 𝑌 𝑥̇𝑆𝑆𝑅 = 𝑢̇ + 𝑌̇
𝑥̈𝑆𝑆𝑅 = 𝑢̈ + 𝑌̈ 
𝑌 = 𝑅(𝜔2𝑡)[𝑅(𝜔1𝑡)(𝑋 − 𝑋𝑂) − 𝑋𝐶] + 𝑌𝑇(𝑡) 
where R is the rotation matrix obtained by integrating the appropriate angular velocity,  
the magnitude of the angular velocities 𝜔1 and 𝜔2 are defined by load curves LCD1 and 
LCD2  respectively,  and  the  directions  are  defined  by  the  current  coordinates  of  the 
node  pairs  N1-N2  and  N3-N4  .    The  velocity  corresponding  to  the 
translational term, YT(t),  is defined in magnitude by LCD3 and in direction by the node 
pair  N5-N6.    The  initial  coordinates  of  the  nodes  are  X,  XO  is  the  initial  coordinate 
vector of node N1 and XC is the initial coordinate vector of node N3.  If data defining an 
angular velocity is not specified, the velocity is defaulted to zero, and R is the identity 
matrix.  In a similar manner, if the translational velocity is not specified, it is defaulted 
to zero. 
This capability is useful for initializing the stresses and velocity of tires during dynamic 
relaxation, and rolling processes in manufacturing.  It is available for solid formulations 
1,  2,  10,  13,  and  15,  and  for  shell  formulations  2,  4,  5,  6,  16,  25,  26,  and  27.    It  is  not 
available for beams and tshells.  It is available for implicit and explicit simulations and 
is  invoked  for  dynamic  relaxation  by  specifying  that  the  load  curves  are  used  during 
dynamic relaxation.  At the end of the dynamic relaxation, the velocities of the parts are 
set to 𝑥̇𝑆𝑆𝑅and the remaining parts are initialized according to the input file.   
Users must ensure that the appropriate load curves are turned on during the relaxation 
process,  and  if  implicit  dynamic  relaxation  is  used,  that  sufficient  constraints  are 
applied  during  the  initialization  to  remove  any  rigid  body  motion  and  that  they  are 
removed at the end of the dynamic relaxation.  The implicit iteration convergence rate is 
often  improved  by  adding  the  geometric  stiffness  matrix  using  *CONTROL_IMPLIC-
IT_GENERAL.  A consistent tangent matrix is available by using *CONTROL_IMPLIC-
IT_GENERAL,  and  while  it  improves  the  convergence  rate  with  problems  with  small 
strains, it is often unstable for problems with large strains.  The *CONTROL_STEADY_-
STATE_ROLLING  options  should  be  used  to  ramp  up  the  frictional  forces  to  obtain 
smooth solutions and good convergence rates.  
To obtain the free-rolling angular velocity, the tire should be first inflated, then brought 
into contact with the road while the frictional force is ramped up with a load curve and 
a  large  value  of  SCL_K  specified  in  *CONTROL_STEADY_STATE_ROLLING.    The 
angular velocity of the tire is then slowly varied over a range that covers the free rolling 
velocity.    The  free  rolling  velocity  is  obtained  when  either  the  frictional  force  in  the 
direction  of  rolling  or  the  moment  about  the  tire  axis  is  near  zero.    For  a  tire  with  an
initial radius of R and a translational velocity of V, the approximate value for the free 
rolling value of the rolling velocity is 𝜔 = 𝑉
(1+𝜀)𝑅, where 𝜀 is the hoop strain of the rolling 
tire.  For a first guess, the hoop strain can be set to 0.0, and the rolling velocity will be 
within 10% of the actual value.  After the first calculation, a smaller range bracketing the 
free  rolling  velocity  should  be  used  in  a  second  calculation  to  refine  the  free  rolling 
velocity.    An  accurate  value  of  the  free  rolling  velocity  is  necessary  for  subsequent 
analyses, such as varying the slip angle of the tire. 
A  time  varying  slip  angle  can  be  specified  by  moving  one  of  the  nodes  defining  the 
direction vector of the translational velocity.  To check that the stiffness  scale factor in 
*CONTROL_STEADY_STATE_ROLLING is high enough, a complete cycle from a zero 
slip angle to a maximum value, then back to zero, should be performed.  If the loading 
and unloading values are reasonably close, then the stiffness scale factor is adequate.
Available options include: 
<BLANK> 
SET 
*LOAD_STIFFEN_PART 
Purpose:  Staged construction.  Available for solid, shell, and beam elements. 
Note:  This keyword card is available starting in release 3 of version 971. 
Id  Cards.    Include  as  many  of  these  cards  as  desired.    This  input  ends  at  the  next 
keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID/PSID 
LC 
(blank) 
STGA 
STGR 
Type 
I 
Default 
none 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
Part ID (or Part Set ID for the_SET option) 
Load curve defining factor vs.  time 
Construction stage at which part is added (optional) 
Construction stage at which part is removed (optional) 
PID 
LC 
STGA 
STGR 
Remarks: 
1. 
In  many  cases  it  is  more  convenient  to  use  *DEFINE_STAGED_CONSTRUC-
TION_PART which automatically generates *LOAD_STIFFEN_PART data. 
2.  For  parts  that  are  initially  present  but  are  excavated  (removed)  during  the 
analysis, the stiffness factor starts at 1.0.  During the excavation time, it ramps 
down to a small value such as 1.0E-6.  The excavation time should be sufficient-
ly long to avoid introducing shock or dynamic effects.  For parts that are intro-
duced  during  the  construction,  e.g.    retaining  walls,  the  elements  are  initially 
present in the model but the factor is set to a low value such as 1.0e-6.  During
the construction time the factor should be ramped up to 1.0.  The construction 
time should be sufficiently long to avoid shock or dynamic effects.  A factor that 
ramps up from 1.0E-6 to 1.0, then reduces back to 1.0E-6, can be used for tem-
porary retaining walls, props, etc. 
3.  When the factor is increasing, it applies only to the stiffness and strength of the 
material in response to subsequent strain increments, not to any existing stress-
es. 
4.  When the factor is decreasing, it applies also to existing stresses as well as to the 
stiffness and strength. 
5.  This  feature  works  with  all  material  models  when  used  only  to  reduce  the 
stiffness  (e.g.    parts  that  are  excavated,  not  parts  that  are  added  during  con-
struction).  It works for most material types in all other cases, except those few 
materials  that  re-calculate  stresses  each  time  step  from  total  strains  (elastic, 
SOIL_BRICK, rubber models, orthotropic elastic, fabric, etc).  There is no error 
check  at  present  to  detect  STIFFEN_PART  being  used  with  an  inappropriate 
material model.  Symptoms of resulting problems would include non-physical 
large  stresses  when  a  part  stiffens,  due  to  the  accumulated  strains  in  the 
“dormant” material since the start of the analysis. 
6.  This feature is generally used with *LOAD_GRAVITY_PART.  The same curve 
is often used for the stiffness factor and the gravity factor. 
7.  There are 3 methods of defining the factor-versus-time: 
a)  LC overrides all the other methods if non-zero 
b)  STGA, STGR refer to stages at which the part is added and removed – the 
stages  are  defined  in  *DEFINE_CONSTRUCTION_STAGES.    If  STGA  is 
zero, the part has full  stiffness at time zero.  If not, it ramps up from the 
small  factor  FACT  (on  *CONTROL_STAGED_CONSTRUCTION)  up  to 
1.0  over  the  ramp  time  at  the  start  of  stage  STGA.    If  STGR  is  zero,  the 
stiffness  factor  continues  at  1.0  until  the  end  of  the  analysis.    If  not,  it 
ramps  down  from  1.0  to  FACT  over  the  ramp  time  at  the  start  of  stage 
STGR. 
c)  *DEFINE_STAGED_CONSTRUCTION_PART  can  be  used  instead  of 
*LOAD_STIFFEN_PART  to  define  this  loading.    During  initialization,  a 
*LOAD_STIFFEN_PART card will be created and the effect is the same as 
using the STGA, STGR method described above.
*LOAD_SUPERPLASTIC_FORMING 
Purpose:    Perform  superplastic  forming  (SPF)  analysis.    This  option  can  be  applied  to 
2D and 3D solid elements and to 3D shell elements, and has been implemented for both 
explicit  and  implicit  analyses.    The  pressure  loading  controlled  by  the  load  curve  ID 
given below is scaled to maintain a constant maximal strain rate or other target value. 
This option must be used with material model 64, *MAT_RATE_SENSITIVE_POWER-
LAW_PLASTICITY,  for  strain  rate  sensitive,  powerlaw  plasticity.    For  the  output  of 
data, see *DATA-BASE_SUPERPLASTIC_FORMING.  Mass scaling is recommended in 
SPF applications. 
New  options  to  compute  the  target  value  with  various  averaging  techniques  and 
autojump  options  to  control  the  simulation  are  implemented.    Strain-rate  speedup  is 
also available.  See Remarks 5-7 for details. 
Card Sets.  Include as many sets consisting of the following four cards as desired.  This 
input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCP1 
CSP1 
NCP1 
LCP2 
CSP2 
NCP2 
PCTS1 
PCTS2 
Type 
I 
I 
F 
I 
I 
F 
F 
F 
Default 
none 
none 
none. 
none 
none 
none 
100.0 
100.0 
Remarks 
  Card 2 
1 
2 
3 
1 
4 
1 
5 
1 
6 
7 
Variable 
ERATE 
SCMIN 
SCMAX 
NCYL 
NTGT 
LEVEL 
TSRCH 
Type 
F 
F 
F 
Default 
none 
none 
none 
Remarks 
27-98 (LOAD) 
I 
0 
2 
I 
1 
I 
0 
5 
F 
none 
0.0 
LS-DYNA R10.0
Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TPEAK 
TNEG 
TOSC 
POSC 
PDROP 
RILIM 
RDLIM 
STR 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
10.0 
5.0 
10.0 
1.0 
2.0 
1.0 
1.0 
0.0 
Remarks 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
Variable 
THRES 
LOWER 
UPPER 
TFACT 
NTFCT 
BOX 
Type 
F 
F 
F 
F 
I 
Default 
5.0 
90.0 
99.0 
1.0 
10 
I 
0 
Remarks 
7 
7 
6 
8 
  VARIABLE   
LCP1 
CSP1 
NCP1 
LCP2 
CSP2 
DESCRIPTION
Load curve number for Phase I pressure loading, 
.    The  scaled  version  of  this  curve  as
calculated by LS-DYNA is output to “curve1”.  See Remark 3. 
Contact surface number to determine completion of Phase I. 
Percent of nodes in contact to terminate Phase I, 
. 
Load curve number for Phase II pressure loading (reverse), 
.    The  scaled  version  of  this  curve  as
calculated by LS-DYNA is output to “curve2”.  See Remark 3. 
Contact surface to determine completion of Phase II, 
. 
NCP2 
Percent of nodes in contact to terminate Phase II.
*LOAD_SUPERPLASTIC_FORMING 
DESCRIPTION
PCTS1 
PCTS2 
ERATE 
SCMIN 
SCMAX 
NCYL 
NTGT 
Percentage  of  nodes-in-contact  to  active  autojump  in  Phase  I 
forming. 
Percentage  of  nodes-in-contact  to  active  autojump  in  Phase  II 
forming. 
Desired target value.  If it’s strain rate, this is the time derivative
of the logarithmic strain. 
Minimum  allowable  value  for  load  curve  scale  factor.    To
maintain a constant strain rate the pressure curve is scaled.  In the
case  of  a  snap  through  buckling  the  pressure  may  be  removed
completely.  By putting a value here the pressure will continue to
act  but  at  a  value  given  by  this  scale  factor  multiplying  the
pressure curve. 
Maximum allowable value for load curve scale factor.  Generally,
it  is  a  good  idea  to  put  a  value  here  to  keep  the  pressure  from
going to unreasonable values after full contact has been attained. 
When full contact is achieved the strain rates will approach zero
and  pressure  will  go  to  infinity  unless  it  is  limited  or  the
calculation terminates. 
Number of cycles for monotonic pressure after reversal. 
Type of the target (controlling) variable: 
EQ.1: strain rate. 
EQ.2: effective stress. 
LEVEL 
Criterion to compute averaged maximum of controlling variable:
EQ.0:  no average used. 
GE.1:  averaging over neighbors of element with peak value of
controlling  variable.    This  parameter  determines  the
level of  neighbor search. 
EQ.-1:  averaging  over elements  within  selective  range  of  peak
controlling variable. 
TSRCH 
Time interval to conduct neighbors search. 
AT 
Time when SPF Phase I simulation starts. 
TPEAK 
Additional  run  time  to  terminate  simulation  when  maximum
pressure is reached.
VARIABLE   
DESCRIPTION
TNEG 
TOSC 
POSC 
PDROP 
Additional  run  time  to  terminate  simulation  when  percentage
change of nodes-in-contact is zero or negative. 
Additional  run  time  to  terminate  simulation  when  percentage
change of nodes-in-contact oscillates within a specific value. 
Percentage  change  to  define  the  oscillation  of  percentage  of
nodes-in-contact. 
Drop  in  percentage  of  nodes-in-contact  from  the  maximum  to 
terminate  simulation  after  the  specified  termination  percentage
has been reached. 
STR 
Autojump  option  or  strike-through  time  (period  of  time  without 
autojump check): 
EQ.0:  no autojump 
EQ.-1:  autojump controlled by peak pressure 
EQ.-2:  autojump controlled by percentage of nodes in contact 
EQ.-3:  autojump controlled by both above 
GT.0:  strike-through time, then same as STR = -3 
THRES 
LOWER 
UPPER 
Threshold percentage that gives the threshold value above which
elements are considered for average. 
Lower  percentile  of  elements  above  the  threshold  value  to  be
included for average. 
Upper  percentile  of  elements  above  the  threshold  value  to  be
included for average. 
RILIM 
Maximum percentage change for pressure increment. 
RDLIM 
Maximum percentage change for pressure decrement. 
TFACT 
Strain rate speedup factor. 
NTFCT 
Number of computing cycles to ramp up speedup. 
BOX 
Box ID or box set ID.  See Remark 8. 
GT.0: box ID, see *DEFINE_BOX. 
    LT.0: |BOX| is box set ID, see *SET_BOX.
*LOAD_SUPERPLASTIC_FORMING 
1.  Optionally, a second phase can be defined.  In this second phase a unique set of 
pressure segments must be defined whose pressure is controlled by load curve 
2.    During  the  first  phase,  the  pressure  segments  of  load  curve  2  are  inactive, 
and likewise, during the second phase the pressure segments of the first phase 
are  inactive.    When  shell  elements  are  used  the  complete  set  of  pressure  seg-
ments can be repeated in the input with a sign reversal used on the load curve.  
When  solid  elements  are  used  the  pressure  segments  for  each  phase  will,  in 
general, must be unique. 
2.  This is an ad hoc parameter which should probably not be used. 
3.  There  are  three  output  files  “pressure”,  “curve1”,  and  “curve2”  from  the  SPF 
simulation, and they may be plotted using ASCII > superpl in LS-PrePost.  The 
file “curve2” is created only if the second phase is active.  The time interval for 
writing  out  these  files  is  controlled  by  *DATABASE_SUPERPLASTIC_FORM-
ING.    The  files  “curve1”  and  “curve2”  contain  the  adjusted  pressure  histories 
calculated  by  SPF  solver.    File  “pressure”  contains  time  histories  of  scaling 
factor, maximal target value, averaged target value, and percentage of contact. 
4.  The constraint method contact, *CONTACT_CONSTRAINT_NODES_TO_SUR-
FACE, is recommended for superplastic forming simulations since the penalty 
methods are not as reliable when mass scaling is applied.  Generally, in super-
plastic  simulations  mass  scaling  is  used  to  enable  the  calculation  to  be  carried 
out in real time. 
5. 
In order to reduce the oscillation in pressure, the maximal target value used to 
adjust the pressure load is calculated by special averaging algorithm.  There are 
two options available: 
a)  Averaging over neighbors of element with maximum target value: In this meth-
od, the element that has the maximum strain rate or other controlling var-
iable is stored in each cycle of the computation.  The elements close to the 
element  with  the  maximum  value  are  searched  and  stored  in  an  array.  
The averaged maximal target value is computed over the neighboring el-
ements.    The  user  can  input  an  integer  number  to  control  the  level  of 
neighbor  search,  which  will  affect  the  total number  of  elements  for  aver-
age.  Because the neighbor search is time consuming, the user can input a 
time interval to limit the occurrence of searching.  The neighbor search is 
conducted only when the simulation time reaches the specified time or the 
element with maximum target value falls out of the array of neighbors. 
b)  Averaging over elements within selective range of target value: In this method, 
all  elements  that  have  target  value  above  a  threshold  value  (a  threshold 
percentage of maximum target value) are sorted according to their target
value  and  the  elements  between  the  user  specified  lower  percentile  and 
upper percentile are selected to compute the average of the maximal tar-
get value. 
6.  The  SPF  simulation  can  be  controlled  by  various  autojump  options.    When 
autojump  conditions  are  met,  the  SPF  simulation  will  be  either  terminated  or 
continued from phase I to phase II simulation.  The autojump check can be held 
inactive  by  setting  a  strikethrough  time.    In  this  case  the  SPF  simulation  will 
continue for that period of time and only be interrupted when the percentage of 
nodes-in-contact  reaches  100%  for  a  specified  time.    The  available  autojump 
conditions are: 
a)  Peak  pressure  is  reached  and  stays  for  certain  time:  The  peak  pressure  is  de-
termined by the maximum allowable scale factor and the load curve.  The 
simulation will continue for a user specified time before termination. 
b)  User specified percentage of nodes-in-contact is reached: The simulation will be 
terminated or continued to Phase II automatically if one of the following 
conditions is met: 
i) 
ii) 
iii) 
iv) 
If the change of the percentage of nodes-in-contact is zero or nega-
tive for a specified time. 
If the percentage of nodes-in-contact oscillates in a specified range 
for a specified time. 
If the percentage of nodes-in-contact drops more than a specified 
value from the maximum value recorded. 
If the percentage of nodes-in-contact reaches a user specified stop 
value. 
7. 
8. 
In  order  to  speed  up  the  simulation  of  the  superplastic  forming  process,  we 
scale  down  the  computation  time.    By  doing  this  we  increase  the  strain  rate 
allowed  in  the  SPF  process,  resulting  in  reduced  simulation  time.    However, 
caution should be utilized with this speedup as it may affect the accuracy of the 
results.    We  recommend  no  or  small  strain  rate  speedup  for  simulations  with 
complex geometry or tight angles. 
If  the  user  knows  the  area(s)  in  the  workpiece  that  are  critical  in  the  SPF 
process, he can use the box option to limit the region(s) where the elements are 
checked for computing the average of the maximal target value.
*LOAD_SURFACE_STRESS_{OPTION} 
Available options include: 
<BLANK> 
SET 
Purpose:    This  keyword  modifies  the  behavior  of  shell  elements  causing  them  to  pass 
pressure-type loads to material models 37 and 125 ; shells usually 
omit such effects. 
With  this  keyword,  LS-DYNA  calculates  segment  pressures  from  contact  and  applied 
pressure  loads  on  both  the  upper  and  lower  surfaces  of  the  shell  and  applies  them  as 
negative local 𝑧-stresses during the simulation.  It is found in some cases this capability 
can improve the accuracy of metal forming simulations. 
Card  Sets.    Include  as  many  sets  consisting  of  the  following  three  cards  as  desired.  
This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID/PSID 
Type 
I 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LSCID1 
LSCID2 
LSCID3 
LSCID4 
LSCID5 
LSCID6 
LSCID7 
LSCID8 
Type 
I 
  Card 3 
1 
I 
2 
I 
3 
I 
4 
I 
5 
I 
6 
I 
7 
I 
8 
Variable 
USCID1 
USCID2 
USCID3 
USCID4 
USCID5 
USCID6 
USCID7 
USCID8 
Type 
I 
I 
I 
I 
I 
I 
I
VARIABLE   
DESCRIPTION
PID/PSID 
Part ID or if option set is active, part set ID. 
Lower surface contact IDs.  Up to eight IDs can be defined.  These
contacts definitions contribute to the pressure acting on the lower
surface of the shell.  If the pressure on the lower surface is due to
applied pressure loads, specify a value -1 instead of a contact ID. 
Only one of the LSCIDn may be set to -1. 
Lower surface of a part is on the opposite side of the shell element
normals, which must be made consistent (in LS-PrePost). 
Upper surface contact IDs.  Up to eight IDs can be defined.  These 
contacts definitions contribute to the pressure acting on the upper
surface of the shell.  .  If the pressure on the upper surface is due
to applied pressure loads, specify a value of -1 instead of a contact 
ID.  Only one of the USCIDn may be set to -1. 
Upper  surface  of  a  part  is  on  the  same  side  of  the  shell  element
normals, which must be made consistent (in LS-PrePost). 
LSCIDn 
USCIDn 
Remarks: 
1.  MAT_TRANSVERSLY_ANISOTROPIC_ELASTIC_PLASTIC 
This 
keyword  can  be  used  with  *MAT_037  when  ETAN  is  set  to  a  negative  value 
, which triggers normal stresses (local 𝑧-stresses) 
resulting either from sliding contact or applied pressure to be considered in the 
shell formulation.  The normal stresses can be significant in male die radius and 
corners  in  forming  of  Advanced  High  Strength  Steels  (AHSS).    The  negative 
local  𝑧-stresses  are  written  to  the  d3plot  files  after  Revision  97158,  and  can  be 
plotted  in  LS-PrePost  by  selecting  𝑧-stress  under  FCOMP  →  Stress  and  select 
local under FCOMP. 
(37). 
2.  MAT_KINEMATIC_HARDENING_TRANSVERSLY_ANISOTROPIC 
(125).  
This  keyword  can  also  be  used  in  a  simulation  with  *MAT_125  to  account  for 
the normal stresses  .  For this material inserting 
this  keyword  anywhere  in  the  input  deck  will  invoke  the  shell  normal  stress 
calculation.
*LOAD_THERMAL_OPTION 
Available options include: 
CONSTANT 
CONSTANT_ELEMENT_OPTION 
CONSTANT_NODE 
LOAD_CURVE 
TOPAZ 
VARIABLE 
VARIABLE_ELEMENT_OPTION 
VARIABLE_NODE 
VARIABLE_SHELL_OPTION 
Purpose:    To  define  nodal  temperatures  that  thermally  load  the  structure.    Nodal 
temperatures defined by the *LOAD_THERMAL_OPTION method are all applied in a 
structural  only  analysis.    They  are  ignored  in  a  thermal  only  or  coupled  ther-
mal/structural analysis, see *CONTROL_THERMAL_OPTION. 
All  the  *LOAD_THERMAL  options  cannot  be  used  in  conjunction  with  each  other.  
Only those of the same thermal load type, as defined below in column 2, may be used 
together. 
*LOAD_THERMAL_CONSTANT 
-  Thermal load type 1 
*LOAD_THERMAL_ELEMENT 
-  Thermal load type 1 
*LOAD_THERMAL_CONSTANT_NODE 
-  Thermal load type 1 
*LOAD_THERMAL_LOAD_CURVE 
-  Thermal load type 2 
*LOAD_THERMAL_TOPAZ 
-  Thermal load type 3 
*LOAD_THERMAL_VARIABLE 
-  Thermal load type 4 
*LOAD_THERMAL_VARIABLE_ELEMENT 
-  Thermal load type 4 
*LOAD_THERMAL_VARIABLE_NODE 
-  Thermal load type 4 
*LOAD_THERMAL_VARIABLE_SHELL 
-  Thermal load type 4
*LOAD 
Purpose:    Define  nodal  sets  giving  the  temperature  that  remains  constant  for  the 
duration  of  the  calculation.    The  reference  temperature  state  is  assumed  to  be  a  null 
state  with  this  option.    A  nodal  temperature  state,  read  in  above  and  held  constant 
throughout  the  analysis,  dynamically  loads  the  structure.    Thus,  the  temperature 
defined  can  also  be  seen  as  a  relative  temperature  to  a  surrounding  or  initial 
temperature. 
Card Sets.  Include as many sets consisting of the following two cards as desired.  This 
input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSID 
NSIDEX 
BOXID 
Type 
I 
I 
Default 
none 
0. 
I 
0. 
3 
4 
5 
6 
7 
8 
  Card 2 
Variable 
Type 
1 
T 
F 
Default 
0. 
2 
TE 
F 
0. 
  VARIABLE   
DESCRIPTION
NSID 
Nodal set ID containing nodes for initial temperature 
EQ.0: all nodes are included: 
NSIDEX 
BOXID 
Nodal  set  ID  containing  nodes  that  are  exempted  from  the
imposed temperature (optional). 
All nodes in box which belong to NSID are initialized.  Others are
excluded (optional). 
T 
Temperature
*LOAD_THERMAL_CONSTANT 
DESCRIPTION
TE 
Temperature of exempted nodes (optional)
*LOAD_THERMAL_CONSTANT_ELEMENT_OPTION 
Available options include: 
BEAM 
SHELL 
SOLID 
TSHELL 
Purpose:  Define a uniform element temperature that remains constant for the duration 
of  the  calculation.    The  reference  temperature  state  is  assumed  to  be  a  null  state.    An 
element  temperature,  read  in  above  and  held  constant  throughout  the  analysis, 
dynamically loads the structure.  The defined temperature can also be seen as a relative 
temperature to a surrounding or initial temperature. 
Element  Cards.    Include  as  many  cards  in  this  format  as  desired.    This  input  ends  at 
the next keyword (“*”) card. 
3 
4 
5 
6 
7 
8 
  Card 1 
1 
Variable 
EID 
Type 
I 
2 
T 
F 
Default 
none 
0. 
  VARIABLE   
DESCRIPTION
Element ID 
Temperature, see remark below. 
EID 
T 
Remarks: 
1.  The  temperature  range  for  the  constitutive  constants  in  the  thermal  materials 
must  include  the  reference  temperature  of  zero.    If  not  termination  will  occur 
with a temperature out-of-range error immediately after the execution phase is 
entered.
*LOAD_THERMAL_CONSTANT_NODE 
Purpose:    Define  nodal  temperature  that  remains  constant  for  the  duration  of  the 
calculation.    The  reference  temperature  state  is  assumed  to  be  a  null  state  with  this 
option.    A  nodal  temperature  state,  read  in  above  and  held  constant  throughout  the 
analysis,  dynamically  loads  the  structure.    Thus,  the  temperature  defined  can  also  be 
seen as a relative temperature to a surrounding or initial temperature. 
Node Cards.  Include as many cards in this format as desired.  This input ends at the 
next keyword (“*”) card. 
3 
4 
5 
6 
7 
8 
Card 
1 
Variable 
NID 
Type 
I 
2 
T 
F 
Default 
none 
0. 
  VARIABLE   
DESCRIPTION
Node ID 
Temperature, see remark below. 
NID 
T 
Remarks: 
1.  The  temperature  range  for  the  constitutive  constants  in  the  thermal  materials 
must  include  the  reference  temperature  of  zero.    If  not  termination  will  occur 
with a temperature out-of-range error immediately after the execution phase is 
entered.
*LOAD 
Purpose:    Temperatures  computed  in  a  prior  thermal-only  analysis  are  used  to  load  a 
mechanical-only analysis.   The rootname of the d3plot database from the thermal-only 
analysis is specified on the execution line of the mechanical-only analysis using T = tpf, 
where tpf is that rootname, e.g., T = d3plot.   
Warnings:   
1.If  using  a  double  precision  LS-DYNA  executable  in  making  the  two  runs,  do  not 
write the d3plot data using 32ieee format in the thermal-only run, i.e., the envi-
ronment variable LSTC_BINARY must not be set.   
2.The rootnames of the d3plot databases from the two runs must not conflict.  Such 
conflict  can  be  avoided,  for  example,  by  using  jobid = jobname  on  the  execution 
line of the second (mechanical-only) run.
*LOAD_THERMAL_LOAD_CURVE 
Purpose:    Nodal  temperatures  will  be  uniform  throughout  the  model  and  will  vary 
according  to  a  load  curve.    The  temperature  at  time = 0  becomes  the  reference 
temperature  for  the thermal  material.   The  reference  temperature  is  obtained  from the 
optional  curve  for  dynamic  relaxation  if  this curve  is  used.    The  load  curve option  for 
dynamic relaxation is useful for initializing preloads. 
Thermal  Load  Curve  Cards.    Include  as  many  cards  in  this  format  as  desired.    This 
input ends at the next keyword (“*”) card. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
LCIDDR 
Type 
I 
Default 
none 
I 
0 
  VARIABLE   
LCID 
DESCRIPTION
Load  curve  ID,  see  *DEFINE_CURVE,  to  define  temperature 
versus time. 
LCIDDR 
An  optional  load  curve  ID,  see  *DEFINE_CURVE,  to  define 
temperature versus time during the dynamic relaxation phase.
*LOAD 
Purpose:  Nodal temperatures will be read in from the TOPAZ3D database.  This file is 
defined on the execution line by the specification: T = tpf, where tpf is a binary database 
file (e.g., T3PLOT).
*LOAD_THERMAL_VARIABLE 
Purpose:    Define  nodal  temperature  using  node  set(s)  and  temperature  vs.    time 
curve(s). 
Card Sets.  Include as many sets consisting of the following two cards as desired.  This 
input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSID 
NSIDEX 
BOXID 
Type 
I 
I 
Default 
none 
0. 
I 
0. 
  Card 2 
Variable 
1 
TS 
Type 
F 
2 
TB 
F 
3 
4 
5 
6 
7 
8 
LCID 
TSE 
TBE 
LCIDE 
LCIDR 
LCIDEDR 
I 
F 
F 
I 
I 
I 
Default 
0. 
0. 
none 
0. 
0. 
none 
none 
none 
Remark 
1 
1 
1 
1 
1 
  VARIABLE   
DESCRIPTION
NSID 
Nodal set ID containing nodes : 
EQ.0: all nodes are included. 
NSIDEX 
BOXID 
Nodal set ID containing nodes that are exempted (optional), 
. 
All nodes in box which belong to NSID are initialized.  Others are
excluded. 
TS 
TB 
Scaled temperature. 
Base temperature.
VARIABLE   
DESCRIPTION
LCID 
TSE 
TBE 
LCIDE 
LCIDR 
Load  curve  ID  that  multiplies  the  scaled  temperature,  . 
Scaled temperature of the exempted nodes (optional). 
Base temperature of the exempted nodes (optional). 
Load  curve  ID  that  multiplies  the  scaled  temperature  of  the
exempted nodes (optional), . 
Load  curve  ID  that  multiplies  the  scaled  temperature  during the
dynamic relaxation phase 
LCIDEDR 
Load  curve  ID  that  multiplies  the  scaled  temperature  of  the
exempted nodes (optional) during the dynamic relaxation phase. 
Remarks: 
1.  The total temperature is defined as  
𝑇 = TB + TS × 𝑓 (𝑡) 
where 𝑓 (𝑡) is the current value of the load curve, TS is the scaled temperature, 
and TB is the base temperature.   
The rate of thermal strain is based on the rate of temperature change.  In other 
words, the thermal load arises from change in total temperature.  Furthermore, 
the  calculation  of  the  thermal  strain  from  the  coefficient  of  thermal  expansion 
depends  on  the  material  model,  and  some  material  models,  e.g.,  *MAT_255, 
may  offer  multiple  options.      Temperature-dependent  material  properties  are 
based on the total temperature.
*LOAD_THERMAL_VARIABLE_BEAM_{OPTION} 
Available options include: 
<BLANK> 
SET 
Purpose:    Define  a  known  temperature  time  history  as  a  function  of  the  section 
coordinates  for  beam  elements.    To  set  the  temperature  for  the  whole  element  see 
*LOAD_THERMAL_VARIABLE_ELEMENT_BEAM. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
EID/SID 
IPOLAR 
Type 
I 
I 
Default 
none 
none 
1 
0 
Temperature Cards.  Include as many cards in the following format as desired.  This 
input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TBASE 
TSCALE 
TCURVE 
TCURDR 
SCOOR 
TCOOR 
Type 
Default 
F 
0 
F 
I 
I 
F 
F 
1.0 
0 
TCURVE
none 
none 
  VARIABLE   
DESCRIPTION
ID 
Load case ID 
EID/SID 
Beam ID or beam set ID 
IPOLAR 
GT.0:  the  coordinates  SCOOR  and  TCOOR  are  given  in  polar
coordinates  
TBASE 
Base temperature
t 
t 
10   
11   
12   
S = -1, T=+1
S=+1, T=+1 
s 
s 
S = -1, T = -1
S=+1, T = -1 
Figure 0-1.  Figure illustrating point ordering. 
  VARIABLE   
DESCRIPTION
TSCALE 
Constant scale factor applied to temperature from curve 
TCURVE 
Curve ID for temperature vs.  time 
TCURDR 
Curve  ID  for  temperature  vs.    time  used  during  dynamic
relaxation 
SCOOR 
Normalized coordinate in local s-direction (-1.0 to +1.0) 
TCOOR 
Normalized coordinate in local t-direction (-1.0 to +1.0) 
Remarks: 
1.  The temperature T is defined as: 
T = TBASE + TSCALE × 𝑓 (𝑡) 
where 𝑓 (𝑡) is the current ordinate value of the curve.  If the curve is undefined, 
then T = TBASE at all times. 
2.  At least four points (four Card 2’s) must be defined in a rectangular grid.  The 
required order of the points is as shown in Figure 0-1.  First, define the bottom 
row of points (most negative t), left to right in order of increasing s.  Then in-
crement t to define the next row of points, left-to-right in order of increasing s, 
and so on.  The s-t axes are in the plane of the beam cross-section with the s-axis 
in the plane of nodes N1, N2, N3 defined in *ELEMENT_BEAM. 
3.  For  the  polar  option,  SCOOR  is  the  non-dimensional  radius  𝑅/𝑅0  where  𝑅0  is 
the  outer  radius  of  the  section;  and  TCOOR  is  defined  as  θ/π,  where  θ  is  the 
angle in radians from the s-axis, defined in the range –π < θ < π. 
4.  Temperatures will be assigned to the integration points by linear interpolation 
from the points defined using this command.
*LOAD_THERMAL_VARIABLE_ELEMENT_OPTION 
Available options include: 
BEAM 
SHELL 
SOLID 
TSHELL 
Purpose:    Define  element  temperature  that  is  variable  during  the  calculation.    The 
reference  temperature  state  is  assumed  to  be  the  temperature  at  time = 0.0  with  this 
option. 
Element Cards.  Include as many cards in the following format as desired.  This input 
ends at the next keyword (“*”) card. 
Card 
1 
Variable 
EID 
Type 
I 
2 
TS 
F 
3 
TB 
F 
4 
5 
6 
7 
8 
LCID 
I 
Default 
none 
0. 
0. 
none 
  VARIABLE   
DESCRIPTION
Element ID 
Scaled temperature 
Base temperature 
Load  curve  ID  defining  a  scale  factor  that  multiplies  the  scaled
temperature as a function of time,  . 
EID 
TS 
TB 
LCID 
Remarks: 
1.  The temperature is defined as: 
𝑇 = TB + TS × 𝑓 (𝑡) 
where 𝑓 (𝑡) is the current value of the load curve, TS is the scaled temperature, 
and TB is the base temperature
*LOAD_THERMAL_VARIABLE_NODE 
Purpose:    Define  nodal  temperature  that  is  variable  during  the  calculation.    The 
reference  temperature  state  is  assumed  to  be  a  null  state  with  this  option.    A  nodal 
temperature state read in and varied according to the load curve dynamically loads the 
structure.    Thus,  the  defined  temperatures  are  relative  temperatures  to  an  initial 
reference temperature. 
Node  Cards.    Include  as  many  cards  in  the  following  format  as  desired.    This  input 
ends at the next keyword (“*”) card. 
Card 
1 
Variable 
NID 
Type 
I 
2 
TS 
F 
3 
TB 
F 
4 
5 
6 
7 
8 
LCID 
I 
Default 
none 
0. 
0. 
none 
  VARIABLE   
DESCRIPTION
NID 
Node ID 
Scaled temperature 
Base temperature 
Load  curve  ID  that  multiplies  the  scaled  temperature,  . 
TS 
TB 
LCID 
Remarks: 
1.  The temperature is defined as: 
𝑇 = TB + TS × 𝑓 (𝑡) 
where 𝑓 (𝑡) is the current value of the load curve, TS is the scaled temperature, 
and TB is the base temperature
*LOAD_THERMAL_VARIABLE_SHELL_{OPTION} 
Available options include: 
<BLANK> 
SET 
Purpose:    Define  a  known  temperature  time  history  as  a  function  of  the  through-
thickness coordinate for the shell elements. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
EID/SID 
Type 
I 
I 
Default 
none 
none 
Temperature Cards.  Include as many cards of this type as desired.  This input ends at 
the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TBASE 
TSCALE 
TCURVE 
TCURDR 
ZCO 
Type 
Default 
F 
0 
F 
1.0 
I 
0 
I 
F 
TCURVE 
-1/+1 
  VARIABLE   
DESCRIPTION
ID 
Load case ID 
EID/SID 
Shell ID or shell set ID 
TBASE 
Base temperature 
TSCALE 
Constant scale factor applied to temperature from curve 
TCURVE 
Curve ID for temperature vs.  time
VARIABLE   
TCURDR 
DESCRIPTION
Curve  ID  for  temperature  vs.    time  used  during  dynamic
relaxation 
ZCO 
Normalized through-thickness coordinate (-1.0 to +1.0) 
Remarks: 
1.  The temperature T is defined as: 
𝑇 = TBASE  + TSCALE ×  𝑓 (𝑡) 
where 𝑓 (𝑡) is the current ordinate value of the curve.  If the curve is undefined, 
then T = TBASE at all times. 
2.  Through-thickness  points  must  be  defined  in  order  of  increasing  ZCO  (-1.0  to 
+1.0).   ZCO=+1.0 is the top surface of the element, i.e.  the element surface in 
the positive outward normal vector direction from the mid-plane. 
3.  At  least  two  points  (two  Card  2’s)  must  be  defined.    Temperatures  will  be 
assigned  in  the  through-thickness  direction  by  linear  interpolation  from  the 
points defined using this command. 
4. 
5. 
If  the  element  has  multiple  in-plane  integration  points,  the  same  temperature 
distribution is used at each in-plane integration point. 
If  a  shell’s  temperature  distribution  is  defined  using  this  card,  any  values 
defined by *LOAD_THERMAL_NODE are ignored for that shell.
*LOAD_VOLUME_LOSS 
Purpose:  To represent the effect of tunneling on surrounding structures, it is common 
to assume that a pre-defined fraction (e.g., 2%) of the volume occupied by the tunnel is 
lost during the construction process.  This feature is available for solid elements only. 
Part Set Cards.  Include as many of these cards as desired.  This input ends at the next 
keyword (“*”) card. 
Card 
1 
2 
3 
Variable 
PSID 
COORD 
LCUR 
Type 
I 
Default 
none 
I 
0 
I 
0 
4 
FX 
F 
1 
5 
FY 
F 
1 
6 
FZ 
F 
1 
7 
8 
PMIN 
FACTOR 
F 
F 
-1.e20 
.01 
  VARIABLE   
DESCRIPTION
PSID 
Part Set ID 
COORD 
Coordinate System ID (default - global coordinate system) 
LCUR 
Curve ID containing volume fraction lost vs.  time 
FX 
FY 
FZ 
Fraction of strain occurring in x-direction 
Fraction of strain occurring in 𝑦-direction 
Fraction of strain occurring in 𝑧-direction 
PMIN 
(Leave blank) 
FACTOR 
Feedback factor 
Remarks: 
Volume  loss  is  modeled  by  a  process  similar  to  thermal  contraction:  if  the  material  is 
unrestrained  it  will  shrink  while  remaining  unstressed;  if  restrained,  stresses  will 
become  more  tensile.    Typically  the  material  surrounding  the  tunnel  offers  partial 
restraint; the volume loss algorithm adjusts the applied “thermal” strains to attempt to 
achieve the desired volume loss.  Optionally, FX, FY and FZ may be defined: these will 
be  treated  as  ratios  for  the  𝑥,  𝑦  and  𝑧  strains;  this  feature  can  be  used  to  prevent 
contraction parallel to the tunnel axis.
The  total  volume  of  all  the  parts  in  the  part  set  is  monitored  and  output  at  the  time-
history  interval  (on  *DATABASE_BINARY_D3THDT)  to  a  file  named  vloss_output.  
This file contains lines of data (time, volume1, volume2, volume3…) where volume1 is the 
total volume of elements controlled by the first *LOAD_VOLUME_LOSS card, volume2 
is the total volume of elements controlled by the second *LOAD_VOLUME_LOSS card, 
etc. 
This  feature  works  only  with  material  types  that  use  incremental  strains  to  compute 
stresses.  Thus, hyperelastic materials (e.g.  MAT_027) are excluded, as are certain foam 
material types (e.g.  MAT_083). 
The  feedback  factor    controls  how  strongly  the  algorithm  tries  to 
impose the desired change of volumetric strain.  The default value is recommended.  If 
the  volumetric  response  appears  noisy  or  unstable,  it  may  be  necessary  to  reduce 
FACTOR.  Alternatively, if the actual volumetric strain changes much more slowly than 
the input curve, it may be necessary to increase FACTOR.
The keyword *MODULE provides a way to load user compiled libraries at runtime, to 
support  user  defined  capabilities  such  as  material  models,  equations  of  state,  element 
formulations, etc.  The following keywords implement this capability: 
*MODULE_LOAD 
*MODULE_PATH 
*MODULE_USE
*MODULE 
Purpose:  Load a dynamic library for user subroutines. 
Card Sets.  Repeat as many sets data cards as desired (cards 1 and 2) to load multiple 
libraries.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MDLID 
Type 
A20 
Default 
none 
TITLE 
A60 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
FILENAME 
C 
none 
  VARIABLE   
DESCRIPTION
MDLID 
Module identification.  A unique string label must be specified. 
TITLE 
Description of the module. 
FILENAME 
File name of the library to be loaded, 80 characters maximum. 
If  the  filename  has  no  path  component,  LS-DYNA  will  search  in 
all  directories  specified  in  *MODULE_PATH  first.    If  not  found 
and  the  filename  starts  with  “+”  (a  plus  sign),  LS-DYNA  will 
continue  to  search  all  directories  specified  in  the  system
environment variable LD_LIBRARY_PATH.
*MODULE_LOAD 
1.  The  MODULE  capability  described  here  and  in  *MODULE_USE  is  still  under 
development  and  is  considered  experimental.    As  such,  it  is  currently  only 
supported in specially compiled executables on Linux systems 
2. 
is 
option 
library 
If  only  one  dynamic 
loaded  and  no  rules  are  required 
(*MODULE_USE), this dynamic library can be specified through the execution 
line 
variable 
  The 
LD_LIBRARY_PATH is also used for searching the dynamic library if the file-
name  starts  with  “+”.    This  execution  line  option  provides  the  support  to  the 
classic user subroutine subroutines without modifying the input deck.
“module = dll”. 
environment 
system
*MODULE_PATH_{OPTION} 
*MODULE_PATH_{OPTION} 
Available options: 
<BLANK> 
RELATIVE 
*MODULE 
LS-DYNA’s default behavior is search for modules in the current working directory.  If 
a  module  file  is  not  found  and  the  filename  has  no  path  component,  LS-DYNA  will 
search in all directories specified on the cards following a *MODULE_PATH keyword.  
Multiple paths can specified using one *MODULE_PATH keyword card, i.e., 
*MODULE_PATH 
Directory_path1 
Directory_path2 
Directory_path3 
Directory  paths  are  read  until  the  next  “*”  card  is  encountered.    A  directory  path  can 
have up to 236 characters.  See Remark 3. 
When  the  RELATIVE  option  is  used,  all  directories  are  relative  to  the  location  of  the 
input  file.    For  example,  if  “i=/home/test/problems/input.k”  is  given  on  the  command 
line, and the input contains 
*MODULE_PATH_RELATIVE
lib 
../lib 
then the two directories /home/test/problems/lib and /home/test/lib will be searched for 
module files. 
Remarks: 
1.  Filenames and pathnames are limited to 236 characters spread over up to three 
80  character  lines.    When  2  or  3  lines  are  needed  to  specify  the  filename  or 
pathname,  end  the  preceding  line  with  "˽+"  (space  followed  by  a  plus  sign)  to 
signal that a continuation line follows.  Note that the "˽+" combination is, itself, 
part of the 80 character line; hence the maximum number of allowed characters 
is 78 + 78 + 80 = 236.
*MODULE_USE 
Purpose:  Define the rules for mapping the user subroutines loaded in dynamic libraries 
to the model.  The rules can be applied to: 
*MAT_USER_DEFINED_MATERIAL_MODELS 
(MAT 41 - 50) 
*MAT_THERMAL_USER_DEFINED 
*EOS_USER_DEFINED 
*SECTION_SOLID 
*SECTION_SHELL 
(MAT T11 - T15) 
(EOS 21 – 30) 
(ELFORM 101 - 105) 
(ELFORM 101-  105) 
and other subroutines in the LS-DYNA user subroutine package. 
LS-DYNA requires that subroutines in modules  be named as if 
they  were  part  of  the  traditional  user  subroutine  framework.    Each  module,  however, 
can contain a complete set of those subroutines, and it is, therefore, possible to import in 
different modules the same subroutines of the same name several times.  Each module 
is, essentially, an independent copy of the traditional user-subroutine framework.  This 
keyword,  *MODULE_USE,  deals  with  namespace  conflicts  by  defining  how  each 
subroutine in the module is presented to the other keywords. 
The rules defined in *MODULE_USE are applied to only one dynamic library. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MDLID 
Type 
A20 
Default 
none
Rule  Cards.    Card  2  defines  rules  for  the  module  specified  in  Card  1.    Include  one 
instance of this card for each subroutine to be mapped.  If two rules conflict, new rules 
override existing rules.  Input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TYPE 
PARAM1 
PARAM2 
Type 
A20 
A20 
A20 
Default 
none 
blank 
blank 
  VARIABLE   
DESCRIPTION
MDLID 
Module identification defined in *MODULE_LOAD. 
TYPE 
Rule type.  See TYPE definitions below. 
PARAM1 
Type dependent parameter. 
PARAM2 
Type dependent parameter. 
User Defined Materials: 
TYPE   
UMAT 
DESCRIPTION
Implements  the  user  material  type  PARAM1  in  the  model  via  a
possibly different type PARAM2 in the dynamic library.  Types in
the  extended  range  from  1001  to  2000  can  be  used  as  material
types  in  the  model.    For  example,  if  PARAM1 = 1001  and 
PARAM2 = 42,  then  model  material  1001  will  use  subroutine
umat42 from this library. 
If PARAM1 is blank and PARAM2 is not, then all user materials
in the model will use the indicated subroutine from this library. 
If  PARAM2  is  blank  and  PARAM1  is  not,  the  material  type
PARAM1  in  the  model  will  use  the  traditional  subroutine  from
this  library.    For  example,  if  PARAM1 = 43  and  PARAM2  is 
blank, then material type 43 in the model will use the subroutine
umat43 from this library 
If  both  PARAM1  and  PARAM2  are  blank,  then  all  user  defined
MATID 
*MODULE_USE 
DESCRIPTION
materials  in  the  model  will  use  the  traditional  subroutines  from
this library (41 → umat41, 42 → umat42, etc). 
Implements  the  user  material  having  ID = PARAM1  via  a 
possibly different material type PARAM2 in the dynamic library.
PARAM2 may be blank if the material type defined in the model
is the same as the one in the dynamic library. 
PARAM1 can be a numerical id or label of the material as defined 
in the model. 
Materials beyond user material models can be overloaded. 
Thermal User Defined Materials: 
TYPE   
TUMAT 
TMATID 
DESCRIPTION
Implements the user thermal material type PARAM1 in the model
(PARAM1 = 11-15) via type PARAM2 in the dynamic library.  See 
type UMAT for the default rules. 
Implements  the  user  thermal  material  having  ID = PARAM1  via 
thermal material type PARAM2 in the dynamic library.  PARAM2
may be blank if the material type defined in the model is the same
as the one in the dynamic library. 
PARAM1 can be a numerical id or label of the thermal material as 
defined in the model. 
Materials beyond user material models can be overloaded.   
User Defined EOS: 
TYPE   
UEOS 
DESCRIPTION
Implements  the  user  EOS  model  PARAM1  in  the  model
(PARAM1 = 21-30)  via  EOS  model  PARAM2  in  the  dynamic
library.  See type UMAT for the default rules. 
User Defined Elements: 
TYPE   
UELEM 
DESCRIPTION
Implements  the  user  element  type  PARAM1  in  the  model
(PARAM1 = 101-105)  via  element  type  PARAM2  in  the  dynamic
library.  See type UMAT for the default rules.
SECTIONID 
*MODULE 
DESCRIPTION
Implements the user element type with section ID = PARAM1 via 
element type PARAM2 in the dynamic library.  PARAM2 may be
blank if the element type defined in the model is the same as the
one in the dynamic library. 
Note:  Solid  element  types  are  mapped  to  subroutine 
usrsld,  and  shell  element  types  are  mapped  to  sub-
routine  usrshl.    These  interfaces  are  documented  in 
dyn21b.f. 
Other User Subroutines: 
TYPE   
DESCRIPTION
The  following  subroutines  implemented  in  the  dynamic
library  are  used  for  the  model.    Any  subroutines  with  the
same  name  in  other  dynamic  libraries,  if  they  exist,  are
ignored. 
UMATFAIL 
matusr_24 
matusr_103 
UFRICTION 
usrfrc 
UWEAR 
UADAP 
UWELDFAIL 
USPH 
UTHERMAL 
ULOAD 
userwear 
useradap 
uadpnorm 
uadpval 
uweldfail 
uweldfail12 
uweldfail22 
hdot 
usrhcon 
usrflux 
ujntfdrv 
loadsetud 
loadud 
UELEMFAILCTL 
LS-DYNA R10.0 
matfailusercontrol
*MODULE_USE 
DESCRIPTION
UMATFPERT 
usermatfpert 
UREBAR 
rebar_bondslip_get_nhisvar 
rebar_bondslip_get_force 
ULAGPOROUS 
lagpor_getab_userdef 
UAIRBAG 
UALE 
UCOUPLE2OTHER 
airusr 
user_inflator 
al2rfn_criteria5 
al2rmv_criteria5 
alerfn_criteria5 
alermv_criteria5 
shlrfn_criteria5 
shlrmv_criteria5 
sldrfn_criteria5 
sldrmv_criteria5 
f3dm9ale_userdef1 
couple2other_boxminmax 
couple2other_comm 
couple2other_dt 
couple2other_extra 
couple2other_getf 
couple2other_givex 
couple2other_reader 
chkusercomm 
usercomm 
usercomm1 
UOUTPUT 
ushout 
Remarks: 
1. 
In order to simplify the development of user defined materials via modules, the 
*MODULE_USE  keyword  can  be  omitted  in  one  special  case.    If  only  a  single 
module library will be used and no remapping of material types is desired, then 
a  *MODULE_LOAD  keyword  may  appear  with  a  single  library  and  no  other 
*MODULE  keywords.    In  this  case,  all  the  user  defined  subroutines  found  in 
this library will be used in the normal way.  For example, if the library contains 
umat41 and umat43, those routines will be used for all materials of type 41 and 
43 respectively, and the *MODULE_USE keyword describing this may be omit-
ted.
*MODULE 
The following examples demonstrate the input for the MODULE keywords: 
*MODULE_PATH 
*MODULE_LOAD 
*MODULE_USE 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Using *MODULE_PATH to define additional directories where  
$  dynamic libraries are saved. 
$ 
$------------------------------------------------------------------------------ 
$ 
*MODULE_PATH 
/home/lsdynauser/lib 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Using *MODULE_LOAD to load all dynamic libraries for this model. 
$ 
$  three libraries are loaded here for demonstration: 
$ 
$  M_LIB: my own library which is under development.  A debug version is built 
$         in my local directory. 
$         it contains: UMAT41, UMAT42, and UMAT45 
$ 
$  LIB_A: a hypoelastic model, provided by a third party, for shell & solid. 
$          it contains UMAT41 only, with an optional FLUID 
$ 
$  LIB_B: contains two material models provided by another company, with 
$         UMAT41: a elasto-plastic model 
$         UMAT45: a hyper-elastic model for rubber 
$ 
$------------------------------------------------------------------------------ 
*MODULE_LOAD 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
M_LIB               My own library 
/my_development_path/mylib_r123_dbg.so 
LIB_A               library from company A 
Lib_hypoelastic.so 
LIB_B               library from company B 
Lib_plastic.so 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Using *MODULE_USE to map to user subroutines 
$ 
$  CASE 1: 
$ 
$  M_LIB is used for UMAT41,UMAT42,UMAT45 in the model, as default 
$  UMAT41 in LIB_A is used for MT=1001 in the model for shell, and MT=1002 for solid 
$  UMAT45 in LIB_B is used for MATID=202, which also happens to hvae MT=1002 
$ 
*MODULE_USE 
M_LIB 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
UMAT
*MODULE_USE 
LIB_A 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
UMAT                1001                41 
UMAT                1002                41 
*MODULE_USE 
LIB_B 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
MATID               202                 45 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$  CASE 2: 
$ 
$  M_LIB is used for UMAT41,UMAT42 as, 
$         MATID=101 with MT=41 
$         MATID=102 with MT=42 
$  UMAT45 in LIB_B is used with different material properties, as, 
$         MATID=201 with MT=1001 
$         MATID=202 with MT=1002 
$         MATID=203 with MT=1003 
$ 
*MODULE_USE 
LIB_B 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
UMAT                                    45 
*MODULE_USE 
M_LIB 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
MATID               101  
MATID               102
*NODE 
*NODE_{OPTION} 
*NODE_MERGE_SET 
*NODE_MERGE_TOLERANCE 
*NODE_RIGID_SURFACE 
*NODE_SCALAR_{OPTION} 
*NODE_THICKNESS 
*NODE_TO_TARGET_VECTOR 
*NODE_TRANSFORM
Available options include: 
<BLANK> 
MERGE 
*NODE 
Purpose:  Define a node and its coordinates in the global coordinate system.  Also, the 
boundary  conditions  in  global  directions  can  be  specified.    Generally,  nodes  are 
assigned to elements; however, exceptions are possible, see remark 2 below.  The nodal 
point ID must be unique relative to other nodes defined in the *NODE section.   
The  MERGE  option  is  usually  applied  to  boundary  nodes  on  disjoint  parts  and  only 
applies  to  nodes  defined  when  the  merge  option  is  invoked.    With  this  option,  nodes 
with  identical  coordinates  are  replaced  during  the  input  phase  by  the  first  node 
encountered that shares the coordinate.   During the merging process a tolerance is used 
to determine whether a node should be merged.   This tolerance can be defined  using 
the  keyword  *NODE_MERGE_TOLERANCE  keyword,  which  is  recommended  over 
the default value.  See the *NODE_MERGE_TOLERANCE input description in the next 
section. 
Node  Cards.    Include  as  many  cards  in  the  following  format  as  desired.    This  input 
ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
Variable 
NID 
Type 
I 
X 
F 
Default 
none 
0. 
Remarks 
Y 
F 
0. 
Z 
F 
0. 
10 
8 
TC 
9 
RC 
F 
F 
0. 
0. 
1 
1 
  VARIABLE   
DESCRIPTION
NID 
Node number 
X 
Y 
Z 
x coordinate 
y coordinate 
z coordinate
VARIABLE   
DESCRIPTION
TC 
Translational Constraint: 
EQ.0: no constraints, 
EQ.1: constrained x displacement, 
EQ.2: constrained y displacement, 
EQ.3: constrained z displacement, 
EQ.4: constrained x and y displacements, 
EQ.5: constrained y and z displacements, 
EQ.6: constrained z and x displacements, 
EQ.7: constrained x, y, and z displacements. 
RC 
Rotational constraint: 
EQ.0: no constraints, 
EQ.1: constrained x rotation, 
EQ.2: constrained y rotation, 
EQ.3: constrained z rotation, 
EQ.4: constrained x and y rotations, 
EQ.5: constrained y and z rotations, 
EQ.6: constrained z and x rotations, 
EQ.7: constrained x, y, and z rotations. 
Remarks: 
1.  Boundary conditions can also be defined on nodal points in a local (or global) 
system  by  using  the  keyword  *BOUNDARY_SPC.    For  other  possibilities  also 
see the *CONSTRAINED keyword section of the manual. 
2.  A  node  without  an  element  or  a  mass  attached  to  it  will  be  assigned  a  very 
small amount of mass and rotary inertia.  Generally, massless nodes should not 
cause  any  problems  but  in  rare  cases  may  create  stability  problems  if  these 
massless  nodes  interact  with  the  structure.    Warning  messages  are  printed 
when massless nodes are found.  Also, massless nodes are used with rigid bod-
ies to place joints, see *CONSTRAINED_EXTRA_NODES_OPTION and *CON-
STRAINED_NODAL_RIGID_BODY.
*NODE_MERGE_SET 
Purpose:    The  MERGE_SET  option  is  applied  to  a  set  of  boundary  nodes  on  disjoint 
part.  With this option, nodes with identical coordinates that are members of any node 
set ID defined by this keyword are replaced during the input phase by one node within 
the set or sets.  Of the nodes sharing the same coordinates, the node chosen is the one 
with  the  smallest  ID.      During  the  merging  process  a  tolerance  is  used  to  determine 
whether a node should be merged.    This tolerance can  be defined using the keyword 
*NODE_MERGE_TOLERANCE  keyword,  which  is  recommended  over  the  default 
value.    See  the  *NODE_MERGE_TOLERANCE  input  description  in  the  next  section.  
Only nodes contained within the specified sets will be merged.  Nodes contained within 
the  set  are  defined  by  the  *NODE  keyword.    With  this  option,  the  keyword  *NODE_-
MERGE is not needed. 
Node  Set  Cards.    Include  as  many  cards  as  desired.    This  input  ends  at  the  next 
keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSID 
Type 
I 
Default 
none 
  VARIABLE   
DESCRIPTION
NSID 
Node set ID containing list of nodes to be considered for merging.
*NODE 
Purpose:    Define  a  tolerance  is  determine  whether  a  node  should  be  merged  for  the 
keyword,  *NODE_MERGE. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TOLR 
Type 
F 
Default 
yes 
  VARIABLE   
TOLR 
Remarks: 
DESCRIPTION
Physical  distance  used  to  determine  whether  to  merge  a  nodal
pair of nearby nodes.  See remark below. 
If the tolerance, TOLR, is undefined or if it is defaulted to zero, a value is computed as: 
TOLR = 10−5 ⋅
XMAX + YMAX + ZMAX − XMIN − YMIN − ZMIN
3 × √NUMNP
where  XMIN,  XMAX,  YMIN,YMAX,  ZMIN,  and  ZMAX  represent  the  minimum  and 
maximum values of the (x,y,z)  nodal point coordinates in the global coordinate system, 
and NUMNP is the number of nodal points.
*NODE_RIGID_SURFACE 
Purpose:  Define a rigid node and its coordinates in the global coordinate system.  These 
nodes are used to define rigid road surfaces and they have no degrees of freedom.  The 
nodal points are used in the definition of the segments that define the rigid surface.  See 
*CONTACT_RIGID_SURFACE.    The  nodal  point  ID  must  be  unique  relative  to  other 
nodes defined in the *NODE section. 
Node  Cards.    Include  as  many  cards  in  the  following  format  as  desired.    This  input 
ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
NID 
Type 
I 
X 
F 
Default 
none 
0. 
Remarks 
Y 
F 
0. 
Z 
F 
0. 
  VARIABLE   
DESCRIPTION
NID 
Node number 
X 
Y 
Z 
x coordinate 
y coordinate 
z coordinate
Available options include: 
<BLANK> 
VALUE 
*NODE 
Purpose:    Define  a  scalar  nodal  point  which  has  one  degree-of-freedom.    The  scalar 
point ID must be unique relative to other nodes defined in the *NODE section. 
Node Card.  Card 1 for no keyword option (option set to <BLANK>).  Include as many 
cards  in  the  following  format  as  desired.    This  input  ends  at  the  next  keyword  (“*”) 
card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
NID 
NDOF 
Type 
I 
I 
Default 
none 
0 
Node  Card.    Card  1  for  the  VALUE  keyword  option.    Include  as  many  cards  in  the 
following format as desired.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
Variable 
NID 
Type 
I 
Default 
none 
2 
X1 
F 
0 
3 
X2 
F 
0 
4 
X3 
F 
0 
5 
6 
7 
NDOF 
I 
0 
  VARIABLE   
DESCRIPTION
NID 
Scalar node ID.
*NODE_SCALAR 
DESCRIPTION
NDOF 
Number of degrees-of-freedom 
EQ.0: fully constrained 
EQ.1: one degree-of-freedom 
EQ.2: two degrees-of-freedom 
EQ.3: three degrees-of-freedom 
XI 
Initial value of Ith degree of freedom.
*NODE_THICKNESS_{OPTION1}_{OPTION2} 
For OPTION1 the available options include: 
<BLANK> 
SET 
For OPTION2 the available options include: 
<BLANK> 
GENERATE 
Purpose:    Define  nodal  thickness  that  overrides  nodal  thickness  otherwise  determined 
via  *SECTION_SHELL,  *PART_COMPOSITE,  or  *ELEMENT_SHELL_THICKNESS.  
The  option  GENERATE  generates  a  linear  thickness  distribution  between  a  starting 
node (or node set) and a ending node (or node set).   
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ID1 
THK 
ID2 
INC 
Type 
I 
F 
I 
I 
Default 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
Node  ID,  or  node  set  ID  if  SET  option  is  active.    If  GENERATE
option is active, ID1 serves as the starting node (or node set). 
Thickness  at  node  ID1,  or  node  set  ID1  if  SET  option  is  active
(ignored if GENERATE option is active). 
Ending node (or node set) if GENERATE option is active. 
Increment in node numbers if GENERATE option is active. 
ID1 
THK 
ID2 
INC 
Remarks: 
When  the  GENERATE  option  is  active,  both  the  starting  and  ending  nodes  (or  node 
sets)  must  have  a  nodal  thickness  as  defined  by  *NODE_THICKNESS  or  NODE_-
THICKNESS_SET.    The  sample  commands  shown  below  create  a  linear  thickness 
distribution between node set 100 and node set 200. 
*SET_NODE_LIST 
100 
1, 15, 39 
*SET_NODE_LIST 
200 
7, 21, 45 
*NODE_THICKNESS_SET 
$ assign thickness of 2.0 to node 1, 15 and 39  
100, 2.0 
*NODE_THICKNESS_SET 
$ assign thickness of 5.0 to node 7, 21 and 45  
200, 5.0 
*NODE_THICKNESS_SET_GENERATE 
$  assign  thickness  of  3.    (=  2.+1.)  to  node  3  (=1+2),  17  (=15+2)  and  41 
(=39+2) 
$  assign  thickness  of  4.    (=  2.+2.)  to  node  5  (=1+4),  19  (=15+4)  and  43 
(=39+4) 
100,, 200, 2
*NODE 
Purpose:  Calculate vector components of the normal distance from the target to a node 
from 
target. 
fitted 
of  a  part  best 
*CONTROL_FORMING_BESTFIT_VECTOR. 
  This  keyword 
is  generated 
the 
to 
Node  Cards.    Include  as  many  cards  in  the  following  format  as  desired.    This  input 
ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
NID 
XDELTA 
YDELTA 
ZDELTA 
Type 
I 
Default 
none 
F 
0. 
F 
0. 
F 
0. 
  VARIABLE   
DESCRIPTION
NID 
Node ID on a part best fitted to the target. 
Difference in X-coordinates of the normal distance from the target
(typically scan data) to a node of a part best fitted to the target.  
Difference in Y-coordinates of the normal distance from the target
(typically scan data) to a node of a part best fitted to the target. 
Difference in Z-coordinates of the normal distance from the target
(typically scan data) to a node of a part best fitted to the target. 
XDELTA 
YDELTA 
ZDELTA 
Remarks: 
1.  This 
keyword 
from 
*CONTROL_FORMING_BESTFIT_VECTOR  and  is  available  starting  from 
Revision 112655.
automatically 
generated 
is
*NODE_TRANSFORM 
Purpose:  Perform a transformation on a node set based on a transformation defined by 
the keyword *DEFINE_TRANSFORMATION. 
Transformation  Cards.    Include  as  many  cards  in  the  following  format  as  desired. 
This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TRSID 
NSID 
Type 
I 
I 
Default 
none 
none 
  VARIABLE   
TRSID 
DESCRIPTION
The  ID  of  the  transformation  defined  under  *DEFINE_TRANS-
FOR-MATION. 
NSID 
Node set ID of the set of nodes to be subject to the transformation.
The  *PARAMETER  family  of  commands  assign  numerical  values  or  expressions  to 
named  parameters.    The  parameter  names  can  be  used  subsequently  in  the  input  in 
place of numerical values. 
*PARAMETER_OPTION 
*PARAMETER_DUPLICATION 
*PARAMETER_EXPRESSION 
*PARAMETER_TYPE
*PARAMETER_{OPTION}_{OPTION} 
The available options are 
<BLANK> 
LOCAL 
MUTABLE 
Purpose:    Define  the  numerical  values  of  parameter  names  referenced  throughout  the 
input file.  The parameter definitions, if used, should be placed at the beginning of the 
input  file  following  *KEYWORD  or  at  the  beginning  of  an  include  file  if  the  LOCAL 
option is specified. 
Parameter Cards.  Include as many cards as necessary.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PRMR1 
VAL1 
PRMR2 
VAL2 
PRMR3 
VAL3 
PRMR4 
VAL4 
Type 
A 
I, F or C 
A 
I, F or C
A 
I, F or C 
A 
I, F or C
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
PRMRn 
PRMRn sets both the nth parameter and its storage type. 
PRMR = T xxxxxxxxx
⏟⏟⏟⏟⏟⏟⏟
9 character name
The first character, “T”, is decoded as follows: 
T.EQ.“R”:  Parameter is a real number 
T.EQ.“I”:  Parameter is an integer 
T.EQ.“C”:  Parameter is a character 
The remaining 9 characters specifiy the name of the parameter.  A
parameter name “time” (case insensitive) is disallowed.  
For  example,  to  define  a  shell  thickness  named,  "SHLTHK",  the
input  “RSHLTHK”,  “R␣␣␣SHLTHK”,  or  “R␣␣SHLTHK␣”  are  all 
equivalent  10  character  strings  (“␣”  is  space).    For  instructions 
regard how to use the variable “SHLTHK” see Remark 1.
Define  the  value  of  the  nth  parameter  as  either  a  real  or  integer 
number, or a character string consistent with preceding definition
for PRMRn. 
*PARAMETER 
  VARIABLE   
VALn 
Remarks: 
1.  Syntax for Using Parameters.  Parameters can be referenced anywhere in the 
input by placing an "&" immediately preceding the parameter name.  If a minus 
sign  “-“  is  placed  directly  before  “&”,  i.e.,  “-&”,  with  no  space  the  sign  of  the 
numerical value will be switched. 
2.  LOCAL  Option.    *PARAMETER_LOCAL  behaves  like  the  *PARAMETER 
keyword with one difference.  A parameter defined by *PARAMETER without 
the  LOCAL  option  is  visible  and  available  at  any  later  point  in  the  input  pro-
cessing.  Parameters defined via the LOCAL versions disappear when the input 
parser  finishes  reading  the  file  in  which  they  appear.   LOCAL  variables  can 
temporarily mask non-LOCAL variables. 
For example, suppose you have the following input files: 
main.k:  
*PARAMETER  
R  VAL1    1.0  
*PARAMETER  
R  VAL2    2.0  
*PARAMETER  
R  VAL3    3.0  
*CONTROL_TERMINATION  
   &VAL1 
*INCLUDE  
file1  
file1:  
*PARAMETER  
R  VAL1    10.0  
*PARAMETER_LOCAL  
R  VAL2    20.0  
*PARAMETER_LOCAL  
R  VAL4    40.0  
*INCLUDE  
file2  
⋮
Then,  inside  file2  we  will  see  VAL1 = 10.0,  VAL2 = 20.0,  VAL3 = 3.0  and 
VAL4 = 40.0.   In  main.k,  after  returning  from  file1,  we  will  see  VAL1 = 10.0, 
VAL2 = 2.0, and VAL3 = 3.0.  VAL4 will not exist.  This allows for include files 
that can set all their own parameters without clobbering the parameters in the 
rest of the input. 
3.  MUTABLE Option for Redefining.  The MUTABLE option is used to indicate 
that  an  integer  or  real  parameter  may  be  redefined  at  some  later  point  in  the 
input  processing  (it  is  ignored  for  character  parameters).    Redefinition  is  al-
lowed  regardless  of  the  setting  of  *PARAMETER_DUPLICATION.    The  MU-
TABLE qualifier must appear on the first definition of the parameter.  It is not 
required on any later redefinition.
*PARAMETER 
Purpose:    The  purpose  is  to  control  how  the  code  behaves  if  a  duplicate  parameter 
definition is found in the input. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DFLAG 
Type 
Default 
I 
1 
  VARIABLE   
DESCRIPTION
DFLAG 
Flag to control treatment of duplicate parameter definitions: 
EQ.1: issue a warning and ignore the new definition (default) 
EQ.2: issue a warning and accept the new definition 
EQ.3: issue an error and ignore (terminates at end of input) 
EQ.4: accept silently 
EQ.5: ignore silently 
Remarks: 
A  LOCAL  variable  appearing  in  a  file,  which  masks  a  non-LOCAL  parameter,  won't 
trigger these actions; however, a LOCAL that masks another LOCAL or a non-LOCAL 
that masks a non-LOCAL will 
Only one *PARAMETER_DUPLICATION card is allowed.  If more than one is found, a 
warning is issued and any after the first are ignored.
*PARAMETER_EXPRESSION_{OPTION} 
The available options are 
<BLANK> 
LOCAL 
MUTABLE 
Purpose:    Define  the  numerical  values  of  parameter  names  referenced  throughout  the 
input  file.    Like  the  *PARAMETER  keyword,  but  allows  for  general  algebraic 
expressions,  not  simply  fixed  values.    The  LOCAL  option  allows  for  include  files  to 
contain their own unique expressions without clobbering the expressions in the rest of 
the input.  See the *PARAMETER keyword. 
Parameter Cards.  Include as many cards as necessary. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PRMR1 
EXPRESSION1 
Type 
A 
Default 
none 
  VARIABLE   
PRMRn 
A 
none 
DESCRIPTION
Define  the  nth  parameter  in  a  field  of  10.    Within  this  field  the
first character must be either an "R" for a real number, "I" for an
integer,  or  “C”  for  a  character  string.    Lower  or  upper  case  for
"I/C/R"  is  okay.    Following  the  type  designation,  define  the 
name  of  the  parameter  using  up  to,  but  not  exceeding  nine
characters.    For  example,  when  defining  a  shell  thickness
named,  "SHLTHK",  both  inputs  "RSHLTHK"  or  "R      SHLTHK"
can  be  used  and  placed  anywhere  in  the  field  of  10.    When
referencing SHLTHK in the input file see Remark 1 below. 
EXPRESSIONn 
General expression which is evaluated, having the result stored
in PRMRn.  The following functions are available: 
sin, cos, tan, csc, sec, ctn, asin, acos, atan, atan2, sinh, cosh, tanh,
asinh, acosh, atanh, min, max, sqrt, mod, abs, sign, int, aint, nint, 
anint,  float,  exp,  log,  log10,  float,  pi,  and  general  arithmetic
expressions involving +, -, *, /, and **.
VARIABLE   
DESCRIPTION
The  standard  rules  regarding  operator  precedence  are  obeyed,
and  nested  parentheses  are  allowed.    The  expression  can 
reference  previously  defined  parameters  (with  or  without  the
leading  &).    The  expression  can  be  continued  on  multiple  lines
simply by leaving the first 10 characters of the continuation line
blank. 
For type “C” parameters, the expression is not evaluated in any 
sense, just stored as a string. 
Remarks: 
1.  Parameters  can  be  referenced  anywhere  in  the  input  by  placing  an  "&" 
immediately  preceding  the  parameter  name.    Expressions  can  be  included  in 
the  input  when  placed  between  brackets  “<>”  as  long  as  the  total  line  length 
does  not  exceed  80  columns  and  fields  are  comma-delimited.    For  example, 
this… 
*parameter 
rterm, 0.2, istates,  80 
*parameter_expression 
rplot,term/(states-30) 
*DATABASE_BINARY_D3PLOT 
&plot 
is equivalent to 
*parameter 
rterm, 0.2, istates,  80 
*DATABASE_BINARY_D3PLOT 
<term/(states-30)>, 
2.  The integer and real properties of constants and parameters are honored when 
evaluating expressions.  So 2/5 becomes 0, but 2.0/5 becomes 0.4. 
3.  The  sign,  atan2,  min,  max,  and  mod  functions  all  take  two  arguments.    The 
others all take only 1. 
4.  Functions that use an angle as their argument, e.g., sin or cos, assume the angle 
is in radians. 
5.  The MUTABLE option is used to indicate that an integer or real parameter may 
be redefined at some later point in the input processing (it is ignored for charac-
Redefinition  is  allowed  regardless  of  the  setting  of 
ter  parameters). 
*PARAMETER_DUPLICATION.  The MUTABLE qualifier must appear on the 
first definition of the parameter.  It is not required on any later redefinition. 
6.  The unary minus has higher precedence than exponentiation, i.e.  the formula -
3**2 will be interpreted as (−3)2 = 9.
*PARAMETER 
*PARAMETER_TYPE  is  a  variation  on  the  *PARAMETER  keyword  command.    In 
addition to its basic function of associating a parameter name (PRMR) with a numerical 
value  (VAL),  the  *PARAMETER_TYPE  command  also  includes  information  (PRTYP) 
about how the parameter is used by LS-DYNA, e.g., as a Part ID or as a segment set ID.   
*PARAMETER_TYPE  is  useful  only  when  (1)  the  parameter  is  used  to  represent  an 
integer  ID  number,  and  (2)  LS-PrePost  is  used  to  combine  two  or  more  models 
(keyword decks) into a larger model. 
Only  by  knowing  how  the  parameter  is  used  by  LS-DYNA  is  LS-PrePost  able  to 
increment the parameter value by the proper “offset” when LS-PrePost combines two or 
more input decks together into a larger deck.  These offsets are necessary so that IDs of 
a certain type, e.g., Part IDs, are not duplicated in the assembled model.  Figure 30-1 (b)  
shows the offset input dialog box of LS-PrePost where offset values for specific ID types 
are assigned. 
Background: 
This  command  is  designed  to  support  workflows  involving  models  that  are  built  up 
from discrete subassemblies created by independent workgroups.  As the subassembly 
models  evolve  through  the  design  process,  Part  IDs,  material  IDs,  etc.    in  the  models 
may change with each design iteration and therefore it is advantageous to parameterize 
those IDs.  In this way, though the parameter values may change, the parameter names 
remain the same.   When the subassembly models are combined by LS-PrePost to create 
a larger model of an assembly or of a complete system, for instance, an aircraft engine 
model,  parameter  values  assigned  using  *PARAMETER_TYPE  are incremented  by the 
proper ID offset value as prescribed when LS-PrePost imports each keyword file.
*PARAMETER_TYPE 
Parameter  Cards.    For  each  parameter  with  type  information,  include  an  additional 
card.  This input ends at the next keyword (“*”) card. 
Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  PRMR 
VAL 
PRTYP 
Type 
A 
I 
A 
Default 
none 
None 
none
Subsystem ID: 3, Name: 
Filename:
Browse
Offset Settings
Import Offset
Import No Offset
Cancel
(a)
Import With Offset
Default Offset
Set
Largest ID
NODE
PART
SECTION
DEFINE_COORD
SET_DISCRETE
SET_PART
SET_SHELL
SET_TSHELL
ELEMENT/S/STRAIN
MAT
DEFINE_CURVE
SET_BEAM
SET_NODE
SET_SEGMENT
SET_SOLID
EOS
More...
Import
Cancel
(b)
Figure 30-1.  (a) the file → import → keyword dialog box; (b) the LS-PrePost
dialog that takes the offset as a function of ID type. 
  VARIABLE   
DESCRIPTION
PRMR 
PRMR must be in the following format 
PRMR = I xxxxxxxxx
⏟⏟⏟⏟⏟⏟⏟
9 character name
The first character is the type indicator and must be set to “I” for
integer.    The  remaining  9  characters  specifiy  the  name  of  the
parameter. 
input
For  example,  to  define  a  part  ID  "WHLPID",  the 
“IWHLPID”,  “I␣␣␣WHLPID”,  or  “I␣␣WHLPID␣”  are  all 
equivalent  10  character  strings  (“␣”  is  space).    For  instructions 
regard how to use the variable “WHLPID” see remark 1. 
VAL 
Define the value of the parameter.  The VAL field must contain an
integer.
VARIABLE   
PRTYP 
DESCRIPTION
Describes,  for  the  benefit  of  LS-PrePost  only,  how  the  parameter 
PRMR  is  used  by  LS-DYNA.    PRTYP  is  ignored  by  LS-DYNA. 
For example, if VAL represents a Part ID, then PRTYP should be
set to “PID”.  Knowing how the parameter is used by LS-DYNA, 
LS-PrePost  can  apply  the  appropriate  offset  to  VAL  when  input
decks are combined using LS-PrePost. 
EQ.NID: 
EQ.NSID: 
EQ.PID: 
EQ.PSID: 
EQ.MID: 
Node ID, 
Node set ID,  
Part ID, 
Part set ID, 
Material ID,  
EQ.EOSID: 
Equation of state ID,  
EQ.BEAMID: 
Beam element ID, 
EQ.BEAMSID:  Beam element set ID, 
EQ.SHELLID: 
Shell element ID, 
EQ.SHELLSID:  Shell element set ID,  
EQ.SOLIDID: 
Solid element ID, 
EQ.SOLIDSID:  Solid element set ID, 
EQ.TSHELLID:  Tshell element ID,  
EQ.TSHELLSID: Tshell element set ID,  
EQ.SSID: 
Segment set ID 
Remarks: 
1.  Parameters  can  be  referenced  anywhere  in  the  input  by  placing  an  "&"  at  the 
first column of its field followed by the name of the parameter without blanks.   
For example if PRMR is set to “I␣␣WHLPID␣” then the appropriate reference is 
“&WHLPID”. 
Example: 
*PARAMETER_TYPE 
I WHLPID  100       PID 
I WHLMID  300       MID 
*PART 
Wheel 
&WHLPID,200,&WHLMID
2. 
*PARAMETER_TYPE is only supported by LS-PrePost 4.1 or later. 
3.  Combining  *INCLUDE_TRANSFORM  with  *PARAMETER_TYPE  is  unsup-
ported.  This will introduce conflicting parameter offset values, and offset val-
ues  specified 
in  *INCLUDE_TRANSFORM  will  override  offset  values 
associated with *PARAMETER_TYPE.
The following keywords are used in this section: 
*PART_{OPTION1}_{OPTION2}_{OPTION3}_{OPTION4}_{OPTION5} 
*PART_ADAPTIVE_FAILURE 
*PART_ANNEAL 
*PART_COMPOSITE_{OPTION} 
*PART_DUPLICATE 
*PART_MODES 
*PART_MOVE 
*PART_SENSOR 
*PART_STACKED_ELEMENTS
*PART_{OPTION1}_{OPTION2}_{OPTION3}_{OPTION4}_{OPTION5} 
For OPTION1 the available options are 
<BLANK> 
INERTIA 
REPOSITION 
For OPTION2 the available options are  
<BLANK> 
CONTACT 
For OPTION3 the available options are  
<BLANK> 
PRINT 
For OPTION4 the available options are 
<BLANK> 
ATTACHMENT_NODES 
For OPTION5 the available options are 
<BLANK> 
AVERAGED 
Options 1, 2, 3, 4, and 5 may be specified in any order on the *PART card. 
Purpose:  Define parts, i.e., combine material information, section properties, hourglass 
type, thermal properties, and a flag for part adaptivity. 
The INERTIA option allows the inertial properties and initial conditions to be defined 
rather  than  calculated  from  the  finite  element  mesh.    This  applies  to  rigid  bodies,  see 
*MAT_RIGID,  only.    The  REPOSITION  option  applies  to  deformable  materials  and  is 
used  to  reposition  deformable  materials  attached  to  rigid  dummy  components  whose 
motion  is  controlled  by  either  CAL3D  or  MADYMO.    At  the  beginning  of  the 
is  automatically 
calculation  each  component  controlled  by  CAL3D/MADYMO 
repositioned to be consistent with the CAL3D/MADYMO input.  However, deformable 
materials  attached  to  these  components  will  not  be  repositioned  unless  this  option  is 
used.
The  CONTACT  option  allows  part  based  contact  parameters  to  be  used  with  the 
automatic contact types a3, 4, a5, b5, a10, 13, a13, 15 and 26, that is 
*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE, 
*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_MORTAR, 
*CONTACT_SINGLE_SURFACE, 
*CONTACT_AUTOMATIC_NODES_TO_SURFACE, 
*CONTACT_AUTOMATIC_BEAMS_TO_SURFACE, 
*CONTACT_AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE, 
*CONTACT_AUTOMATIC_SINGLE_SURFACE, 
*CONTACT_AUTOMATIC_SINGLE_SURFACE_MORTAR, 
*CONTACT_AIRBAG_SINGLE_SURFACE, 
*CONTACT_ERODING_SINGLE_SURFACE, 
*CONTACT_AUTOMATIC_GENERAL. 
The  default  values  to  use  for  these  contact  parameters  can  be  specified  on  the 
*CONTACT input section card. 
The  PRINT  option  allows  user  control  over  whether  output  data  is  written  into  the 
ASCII files MATSUM and RBDOUT.  See *DATABASE_ASCII. 
The  AVERAGED  option  may  be  applied  only  to  parts  consisting  of  a  single  (non-
branching) line of truss elements.  The average strain and strain rate over the length of 
the  truss  elements  in  the  part  is  calculated,  and  the  resulting  average  axial  force  is 
applied to all of the elements in the part.  Truss elements in an averaged part form one 
long continuous “macro-element.”  The time step size for an AVERAGED part is based 
on the total length of the assembled trusses, rather than on the shortest truss.  
Effectively, the truss elements of an AVERAGED part behave as a string under uniform 
tension.    In  an  AVERAGED  part  there  are  no  internal  forces  acting  to  keep  the  nodes 
separated,  and  other  force  contributions  from  the  surrounding  system  must  play  that 
role.  Therefore, the nodes connected to the truss elements should be attached to other 
structural  members.    This  model  is  prototypically  used  for  modeling  cables  in 
mechanical  actuators.   The  AVERAGED  option  can  be  activated  for  all  material  types, 
which are available for truss elements.
Card Sets.  Repeat as many sets data cards as desired (card 1 through 10).  This input 
ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
HEADING 
C 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
SECID 
MID 
EOSID 
HGID 
GRAV 
ADPOPT 
TMID 
Type 
I/A 
I or A10  I or A10 I or A10 I or A10
Default 
none 
none 
none 
0 
0 
I 
0 
I 
0 
I or A10
0 
Inertia Card 1.  Additional Card for the INERTIA option.  See Remarks 2, 3, and 4.  
  Card 3 
Variable 
1 
XC 
Type 
F 
2 
YC 
F 
3 
ZC 
F 
4 
TM 
5 
6 
7 
8 
IRCS 
NODEID 
F 
I 
I 
Inertia Card 2.  Additional Card for the INERTIA option. 
  Card 4 
1 
Variable 
IXX 
2 
IXY 
3 
IXZ 
4 
IYY 
5 
IYZ 
6 
IZZ 
7 
8 
Type 
F 
F 
F 
F 
F
Inertia Card 3.  Additional Card for the INERTIA option. 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VTX 
VTY 
VTZ 
VRX 
VRY 
VRZ 
Type 
F 
F 
F 
F 
F 
F 
Inertial Coordinate System Card.  Optional card required for IRCS = 1 with INERTIA 
option.  Define two local vectors or a local coordinate system ID.  
  Card 6 
Variable 
Type 
Remark 
1 
XL 
F 
1 
2 
YL 
F 
1 
3 
ZL 
F 
1 
4 
5 
6 
7 
8 
XLIP 
YLIP 
ZLIP 
CID 
F 
1 
F 
1 
F 
1 
I 
none 
Reposition Card.  An additional Card is for the REPOSITION option.  
  Card 7 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CMSN 
MDEP  MOVOPT 
Type 
I 
I 
I 
Contact Card.  Additional Card is required for the CONTACT option. 
  Card 8 
Variable 
1 
FS 
Type 
F 
2 
FD 
F 
3 
DC 
F 
4 
VC 
F 
5 
6 
7 
8 
OPTT 
SFT 
SSF 
CPARM8 
F 
F 
F
NOTE:  If FS, FD, DC, and VC are specified they will not be used unless 
FS  is  set  to  a  negative  value  (-1.0)  in  the  *CONTACT  section.  
These frictional coefficients apply only to contact types: 
SINGLE_SURFACE, 
AUTOMATIC_GENERAL, 
AUTOMATIC_SINGLE_SURFACE, 
AUTOMATIC_SINGLE_SURFACE_MORTAR, 
AUTOMATIC_NODES_TO_..., 
AUTOMATIC_SURFACE_..., 
AUTOMATIC_SURFACE_..._MORTAR, 
AUTOMATIC_ONE_WAY_..., 
ERODING_SINGLE_SURFACE 
Default values are input via *CONTROL_CONTACT input. 
Print Card.  An additional Card is required for the PRINT option.  This option applies 
to rigid bodies and provides a way to turn off ASCII output in files rbdout and matsum. 
  Card 9 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PRBF 
Type 
I 
Attachment Nodes Card.  Additional Card required for the ATTACHMENT_NODES 
option.  See Remark 8. 
  Card 10 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ANSID 
Type 
I 
  VARIABLE   
DESCRIPTION
HEADING 
Heading for the part 
PID 
Part identification.  A unique number or label must be specified.
VARIABLE   
DESCRIPTION
SECID 
MID 
EOSID 
HGID 
Section 
See Remark 7. 
identification  defined 
in  a 
*SECTION  keyword.
Material 
See Remark 7. 
identification  defined 
in 
the 
*MAT 
section.
Equation  of  state  identification  defined  in  the  *EOS  section.
Nonzero  only  for  solid  elements  using  an  equation  of  state  to
compute pressure.  See Remark 7. 
Hourglass/bulk  viscosity  identification  defined  in  the  *HOUR-
GLASS Section.  See Remark 7. 
EQ.0: default values are used. 
GRAV 
Flag to turn on gravity initialization according to *LOAD_DENSI-
TY_DEPTH.   
EQ.0: Part  will  be  initialized  only  if  included  in  the  part  set 
PSID in *LOAD_DENSITY_DEPTH. 
EQ.1: Part  will  be  initialized  irrespective  of  PSID  in  *LOAD_
DENSITY_DEPTH. 
ADPOPT 
Indicate  if  this  part  is  adapted  or  not.    : 
LT.0:  𝑟-adaptive remeshing for 2-D solids, |ADOPT| gives the 
load curve ID that defines the element size as a function
of time. 
EQ.0: Adaptive remeshing is inactive for this part ID. 
EQ.1: ℎ-adaptive for 3-D shells. 
EQ.2: 𝑟-adaptive  remeshing  for  2-D  solids,  3-D  tetrahedrons 
and 
3-D EFG. 
EQ.3: Axisymmetric  r-adaptive  remeshing 
for  3-D  solid 
. 
EQ.9: Passive  ℎ-adaptive  for  3-D  shells.    The  elements  in  this 
part will not be split unless their neighboring elements in
other parts need to be split more than one level.
TMID 
*PART 
DESCRIPTION
Thermal  material  property  identification  defined  in  the  *MAT_-
THERMAL Section.  Thermal properties must be specified for all
solid, shell, and thick  shell parts if a thermal or coupled thermal
structural/analysis is being performed.  Discrete elements are not
considered in thermal analyses.  See Remark 7. 
XC 
YC 
ZC 
TM 
Global 𝑥-coordinate of center of mass.  If nodal point, NODEID, is
defined  XC,  YC,  and  ZC  are  ignored  and  the  coordinates  of  the
nodal point, NODEID, are taken as the center of mass. 
Global 𝑦-coordinate of center of mass 
Global 𝑧-coordinate of center of mass 
Translational mass 
IRCS 
Flag for inertia tensor reference coordinate system: 
EQ.0: global inertia tensor, 
EQ.1: local  inertia  tensor  is  given  in  a  system  defined  by  the
orientation vectors. 
NODEID 
Nodal point defining the CG of the rigid body.  This node should 
be included as an extra node for the rigid body; however, this is
not  a  requirement.    If  this  node  is  free,  its  motion  will  not  be
updated  to  correspond  with  the  rigid  body  after  the  calculation
begins. 
IXX 
IXY 
IXZ 
IYY 
IYZ 
IZZ 
VTX 
𝐼𝑥𝑥, 𝑥𝑥 component of inertia tensor  
𝐼𝑥𝑦,, 𝑥𝑦 component of inertia tensor  
𝐼𝑥𝑧, 𝑥𝑧 component of inertia tensor  
𝐼𝑦𝑦, 𝑦𝑦 component of inertia tensor  
𝐼𝑦𝑧, 𝑦𝑧 component of inertia tensor  
𝐼𝑧𝑧, 𝑧𝑧 component of inertia tensor  
initial  translational  velocity  of  rigid  body  in  global  𝑥  direction
VARIABLE   
DESCRIPTION
VTY 
VTZ 
VRX 
VRY 
VRZ 
XL 
YL 
ZL 
XLIP 
YLIP 
ZLIP 
CID 
initial  translational  velocity  of  rigid  body  in  global  𝑦  direction 
 
initial  translational  velocity  of  rigid  body  in  global  𝑧  direction 
 
initial  rotational  velocity  of  rigid  body  about  global  𝑥  axis 
 
initial  rotational  velocity  of  rigid  body  about  global  𝑦  axis 
 
initial  rotational  velocity  of  rigid  body  about  global  𝑧  axis 
 
𝑥-coordinate of local 𝑥-axis.  Origin lies at (0, 0, 0). 
𝑦-coordinate of local 𝑥-axis 
𝑧-coordinate of local 𝑥-axis 
𝑥-coordinate of vector in local 𝑥-𝑦 plane 
𝑦-coordinate of vector in local 𝑥-𝑦 plane 
𝑧-coordinate of vector in local 𝑥-𝑦 plane 
Local  coordinate  system  ID,  see  *DEFINE_COORDINATE_… 
With this option leave fields 1 - 6 blank. 
CMSN 
CAL3D  segment  number /  MADYMO  system  number.    See  the 
numbering in the corresponding program. 
MDEP 
MADYMO ellipse/plane number: 
GT.0:  ellipse number, 
EQ.0: default, 
LT.0:  absolute value is plane number.
MOVOPT 
FS 
FD 
DC 
VC 
*PART 
DESCRIPTION
Flag  to  deactivate  moving  for  merged  rigid  bodies,  see  *CON-
STRAINED_RIGID_BODIES.    This  option  allows  a  merged  rigid 
body  to  be  fixed  in  space  while  the  nodes  and  elements  of  the
generated CAL3D/MADYMO parts are repositioned: 
EQ.0: merged rigid body is repositioned, 
EQ.1: merged rigid body is not repositioned. 
Static coefficient of friction.  The functional coefficient is assumed
to  be  dependent  on  the  relative  velocity  𝑣relof  the  surfaces  in 
contact, 
𝜇𝑐 = FD + (FS − FD)𝑒−DC×∣𝑣rel∣. 
For mortar contact 𝜇𝑐 = FS, i.e., dynamic effects are ignored. 
Dynamic  coefficient  of  friction.    The  functional  coefficient  is
assumed  to  be  dependent  on  the  relative  velocity  𝑣rel  of  the 
surfaces in contact 
𝜇𝑐 = FD + (FS − FD)𝑒−DC×∣𝑣𝑟𝑒𝑙∣. 
For mortar contact 𝜇𝑐 = FS, i.e., dynamic effects are ignored. 
Exponential  decay  coefficient.    The  functional  coefficient  is
assumed  to  be  dependent  on  the  relative  velocity  vrel  of  the 
surfaces in contact 
𝜇𝑐 = FD + ( FS − FD)𝑒−DC×∣𝑣rel∣. 
For mortar contact 𝜇𝑐 = FS (dynamical effects are ignored). 
Coefficient  for  viscous  friction.    This  is  necessary  to  limit  the 
friction force to a maximum.  A limiting force is computed by, 
𝐹lim = VC × 𝐴cont, 
where  𝐴cont  is  the  area  of  the  segment  contacted  by  the  node  in
contact.    The  suggested  value  for  VC  is  to  use  the  yield  stress  in 
shear  VC =
  where  𝜎0  is  the  yield  stress  of  the  contacted 
𝜎𝑜
√3
material. 
OPTT 
Optional  contact  thickness.    This  applies  to  solids,  shells  and
beams.
VARIABLE   
DESCRIPTION
SFT 
SSF 
Optional thickness scale factor for PART ID in automatic contact
(scales  true  thickness).    This  option  applies  only  to  contact  with
shell  elements.    True  thickness  is  the  element  thickness  of  the
shell elements. 
Scale  factor  on  default  slave  penalty  stiffness  for  this  PART  ID
whenever it appears in the contact definition.  If zero, SSF is taken
as unity. 
CPARM8 
Flag  to  exclude  beam-to-beam  contact  from  the  same  PID  for 
CONTACT_AUTOMATIC_GENERAL. 
  This  applies  only  to 
MPP.    Global  default  may  be  set  using  CPARM8  on  *CON-
TACT_…_MPP Optional Card. 
EQ.0: Flag is not set (default). 
EQ.1: Flag is set. 
EQ.2: Flag  is  set.    CPARM8 = 2  has  the  additional  effect  of 
permitting contact treatment of spot weld (type 9) beams 
in  AUTOMATIC_GENERAL  contacts;  spot  weld  beams 
are  otherwise  disregarded  entirely  by  AUTOMATIC_-
GENERAL contacts. 
PRBF 
Print flag for rbdout and matsum files. 
EQ.0: default  is  taken  from  the  keyword  *CONTROL_OUT-
PUT. 
EQ.1: write data into rbdout file only 
EQ.2: write data into matsum file only 
EQ.3: do not write data into rbdout and matsum
Attachment  node  set  ID.    See  Remark  8.    This  option  should  be 
used  very  cautiously  and  applies  only  to  rigid  bodies.    The 
attachment  point  nodes  are  updated  each  cycle  whereas  other
nodes in the rigid body are updated only in the output databases.
All  loads  seen  by  the  rigid  body  must  be  applied  through  this
nodal subset or directly to the center of gravity of the rigid body. 
If the rigid body is in contact this set must include all interacting
nodes. 
EQ.0: All  nodal  updates  are  skipped  for  this  rigid  body.    The
null option can be used if the rigid body is fixed in space
or  if  the  rigid  body  does  not  interact  with  other  parts,
e.g., the rigid body is only used for some visual purpose.
*PART 
  VARIABLE   
ANSID 
Remarks: 
1.  Local  Inertia  Tensor  Coordinate  System.    The  local  Cartesian  coordinate 
system  is  defined  as  described  in  *DEFINE_COORDINATE_VECTOR.    The 
local  𝑧-axis  vector  is  the  vector  cross  product  of  the  𝑥-axis  and  the  in-plane 
vector.  The local 𝑦-axis vector is finally computed as the vector cross product of 
the 𝑧-axis vector and the 𝑥-axis vector.  The local coordinate system defined by 
CID  has  the  advantage  that  the  local  system  can  be  defined  by  nodes  in  the 
rigid body which makes repositioning of the rigid body in a preprocessor much 
easier since the local system moves with the nodal points. 
2. 
3. 
4. 
Inertia Option and Shared Rigid/Deformable Nodes.  When specifying mass 
properties  for  a  rigid  body  using  the  inertia  option,  the  mass  contributions  of 
deformable bodies to nodes which are shared by the rigid body should be con-
sidered as part of the rigid body. 
Inertia  Option  Lacks  Default  Values.    If  the  inertia  option  is  used,  all  mass 
and inertia properties of the body must be specified.  There are no default values. 
Inertia  Tensor  Characteristics.    The  inertia  terms  are  always  with  respect  to 
the  center of  mass  of  the  rigid  body.   The  reference  coordinate  system  defines 
the  orientation  of  the axes,  not the  origin.  Note that  the  off-diagonal  terms  of 
the inertia tensor are opposite in sign from the products of inertia. 
5. 
Initial  Velocity  Card  for  Rigid  Bodies.    The  initial  velocity  of  the  rigid  body 
may be overwritten by the *INITIAL_VELOCITY card.
6.  Axisymmetric  Remeshing.    Axisymmetric  remeshing  is  specially  for  3-D 
orbital forming.  The adaptive part using this option needs to meet the follow-
ing requirement in both geometry and discretization:  
a)  The geometry is (quasi-) symmetric with respect to the local 𝑧-axis, which 
in  turn  must  be  parallel  to  the  global  𝑧-axis.    See  CID  in  *CONTROL_-
REMESHING. 
b)  A set of 2-D cross-sections with uniform angular interval around 𝑧-axis are 
discretized  by  mixed  triangular  and  quadrilateral  elements  in  a  similar 
pattern. 
c)  A  set  of  circular  lines  around 𝑧-axis  pass  through  the  nodes  of  the  cross-
sections and form orbital pentahedrons and hexahedrons. 
7.  Allowed  ID  Values.    The  variables  SID,  MID,  EOSID,  HGID,  and  TMID  in 
*PART,  and  in  *SECTION,  *MAT,  *EOS,  *HOURGLASS,  and  *MAT_THER-
MAL, respectively, may be input as an 10-character alphanumeric variable (20-
characters if long format is used), e.g., “HS Steel”, or as an integer not to exceed 
232 − 1, e.g.,“123456789” is allowed. 
8.  Attachment Nodes Option.  All nodes are treated as attachment nodes if this 
option is not used.  Attachment nodes apply to rigid bodies only.  The motion 
of  these  nodes,  which  must  belong  to  the  rigid  body,  are  updated  each  cycle.  
Other  nodes  in  the  rigid  body  are  updated only  for  output  purposes.    Include 
all nodes in the attachment node set which interact with the structure through 
joints, contact, merged nodes, applied nodal point loads, and applied pressure.  
Include  all  nodes  in  the  attachment  node  set  if  their  displacements,  accelera-
tions,  and  velocities  are  to  be  written  into  an  ASCII  output  file.    Body  force 
loads are applied to the c.g.  of the rigid body.
*PART_ADAPTIVE_FAILURE 
Purpose:  This is an option for two-dimensional adaptivity to allow a part that is singly 
connected  to  split  into  two  parts.    This  option  is  under  development  and  will  be 
generalized in the future to allow the splitting of parts that are multiply connected. 
3 
4 
5 
6 
7 
8 
  Card 1 
1 
Variable 
PID 
Type 
I 
2 
T 
F 
  VARIABLE   
DESCRIPTION
PID 
T 
Part ID 
Thickness.  When the thickness of the part reaches this minimum
value the part is split into two parts.  The value for T should be on 
the order of the element thickness of a typical element.
Available options include: 
<BLANK> 
SET 
*PART 
Purpose:    To  initialize  the  stress  states  at  integration  points  within  a  specified  part  to 
zero  at  a  given  time  during  the  calculation.    This  option  is  valid  for  parts  that  use 
constitutive  models  where  the  stress  is  incrementally  updated.    This  option  applies  to 
the Hughes-Liu beam elements, the integrated shell elements, thick shell elements, and 
solid elements.  In addition to the stress tensor components, the effective plastic strain is 
also set to zero. 
Part  Cards.    Include  as  many  parts  cards  as  desired.    This  input  ends  at  the  next 
keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID/PSID 
TIME 
Type 
I 
F 
Default 
none 
none 
  VARIABLE   
DESCRIPTION
PID/PSID 
Part ID or part set ID if the SET option is active. 
TIME 
Time when the stress states are reinitialized.
*PART_COMPOSITE_{OPTION} 
Available options include: 
<BLANK> 
CONTACT 
TSHELL 
LONG 
Purpose:    The  following  input  provides  a  simplified  method  of  defining  a  composite 
material model for shell elements and thick shell elements that eliminates the need for 
user  defined  integration  rules  and  part  ID’s  for  each  composite  layer.   When  *PART_-
COMPOSITE  is  used,  a  section  definition,  *SECTION_SHELL  or  *SECTION_TSHELL, 
and integration rule definition, *INTEGRATION_SHELL, are unnecessary. 
The  material  ID,  thickness,  material  angle  and  thermal  material  ID  for  each  through-
thickness integration point of a composite shell or thick shell are provided in the input 
for this command.  The total number of integration points is determined by the number 
of entries on these cards. 
Unless the *ELEMENT_SHELL_THICKNESS card is set, the thickness is assumed to be 
constant on each shell element.  The thickness, then, is given by summing the THICK𝑖 
values from card 4 below over the integration points 𝑖.  When the *ELEMENT_SHELL_-
THICKNESS  card  is  included  the  THICK𝑖  values  are  scaled  to  fit  the  nodal  thickness 
values  assigned  using  the  *ELEMENT__SHELL_THICKNESS  keyword.    For  thick 
shells,  the  total  thickness  is  obtained  from  the  positions  of  the  nodes  on  the  top  and 
bottom  surfaces.    In  this  case,  the  THICKi,  are  also  scaled  to  conform  to  the  geometry 
defined by the element’s nodes. 
For  a  more  general  method  of  defining  composite  shells  and  thick  shells,  see  *ELE-
MENT_SHELL_COMPOSITE 
  These 
commands permit unique layer stack-ups for each element without requiring a unique 
part ID for each element. 
*ELEMENT_TSHELL_COMPOSITE. 
and 
With  *PART_COMPOSITE,  two  integration  points  with  4  constants  each  are  provided 
in each Integration Point Properties Card.  On the other hand, with *PART_COMPOS-
ITE_LONG,  for  each  integration  point  there  is  one  Integration  Point  Properties  Card 
containing up to 8 constants. 
To  maintain  a  direct  association  of  through-thickness  integration  point  numbers  with 
physical plies in the case where plies span over more than one part ID, see Remark 5.
The  CONTACT  option  allows  part  based  contact  parameters  to  be  used  with  the 
automatic  contact  types  a3,  4,  a5,  a10,  13,  a13,  15  and  26,  which  are  listed  under  the 
*PART definition above. 
Card  Sets.    Repeat  as  many  sets  data  cards  as  desired.    This  input  ends  at  the  next 
keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
HEADING 
C 
none 
Thin Shell Card.  The following card is required for thin shell composites.  Omit this 
card if the TSHELL option is used.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
ELFORM 
SHRF 
NLOC 
MAREA 
HGID 
ADPOPT 
THSHEL 
Type 
I 
Default 
none 
I 
0 
F 
F 
F 
1.0 
0.0 
0.0 
I 
0 
I 
0 
I 
0 
Thick Shell Card.  This is an additional card for the TSHELL option.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
ELFORM 
SHRF 
HGID 
TSHEAR 
Type 
I 
Default 
none 
I 
0 
F 
1.0 
I 
0 
I
Contact Card.  Additional Card is required for the CONTACT option. 
  Card 3 
Variable 
1 
FS 
Type 
F 
2 
FD 
F 
3 
DC 
F 
4 
VC 
F 
5 
6 
7 
8 
OPTT 
SFT 
SSF 
F 
F 
F 
 NOTE:  If FS, FD, DC, and VC are specified they will not be used unless 
FS  is  set  to  a  negative  value  (-1.0)  in  the  *CONTACT  section.  
These frictional coefficients apply only to contact types: 
SINGLE_SURFACE, 
AUTOMATIC_GENERAL, 
AUTOMATIC_SINGLE_SURFACE, 
AUTOMATIC_NODES_TO_..., 
AUTOMATIC_SURFACE_..., 
AUTOMATIC_ONE_WAY_..., 
ERODING_SINGLE_SURFACE 
Default values are input via *CONTROL_CONTACT input. 
Integration Point Data Cards without Long Option.  The material ID, thickness, and 
material  angle  for  each  through-thickness  integration  point  of  a  composite  shell  are 
provided  below  (up  to  two  integration  points  per  card).    The  integration  point  data 
should be given sequentially starting with the bottommost integration point.  The total 
number  of  integration  points  is  determined  by  the  number  of  entries  on  these  cards. 
Include as many cards as necessary.  The next “*” card terminates this input.  
  Card 4 
1 
2 
Variable 
MID1 
THICK1 
Type 
I 
F 
3 
B1 
F 
4 
5 
6 
TMID1 
MID2 
THICK2 
I 
I 
F 
7 
B2 
F 
8 
TMID2
Integration  Point  Data  Cards  for  Long  Option.    The  material  ID,  thickness,  and 
material  angle  for  each  through-thickness  integration  point  of  a  composite  shell  are 
provided below (one integration point per card).  The integration point data should be 
given sequentially starting with the bottommost integration point.  The total number of 
integration  points  is  determined  by  the  number  of  entries  on  these  cards.    Include  as 
many cards as necessary.  The next “*” card terminates this input.  
  Card 4 
1 
2 
Variable 
MID1 
THICK1 
Type 
I 
F 
3 
B1 
F 
4 
5 
6 
7 
8 
TMID1 
PLYID1 
SHRFAC 
I 
I 
F 
  VARIABLE   
DESCRIPTION
HEADING 
Heading for the part 
PID 
Part ID 
ELFORM 
Element formulation options for thin shells: 
EQ.1:  Hughes-Liu, 
EQ.2:  Belytschko-Tsay, 
EQ.3:  BCIZ triangular shell, 
EQ.4:  C0 triangular shell, 
EQ.6:  S/R Hughes-Liu, 
EQ.7:  S/R co-rotational Hughes-Liu, 
EQ.8:  Belytschko-Leviathan shell, 
EQ.9:  Fully integrated Belytschko-Tsay membrane, 
EQ.10:  Belytschko-Wong-Chiang, 
EQ.11:  Fast (co-rotational) Hughes-Liu, 
EQ.16:  Fully integrated shell element (very fast), 
Element formulation options for thick shells: 
EQ.1:  one point reduced integration, 
EQ.2:  selective reduced 2 x 2 in plane integration, 
EQ.3:  assumed strain 2 x 2 in plane integration,
SHRF 
NLOC 
*PART_COMPOSITE 
DESCRIPTION
EQ.5:   assumed strain reduced integration with brick materials
EQ.6: :  assumed strain reduced integration with shell materials
EQ.7:  assumed strain 2x2 in plane integration 
Shear correction factor which scales the transverse shear stress. 
Location  of  reference  surface,  available  for  thin  shells  only.    If
nonzero, the offset distance from the plane of the nodal points to
the  reference  surface  of  the  shell  in  the  direction  of  the  shell
normal vector is a value: 
offset = −0.50 × NLOC × (average  shell  thickness). 
This  offset  is  not  considered  in  the  contact  subroutines  unless
CNTCO  is  set  to  1  in  *CONTROL_SHELL.    Alternatively,  the 
offset  can  be  specified  by  using  the  OFFSET  option  in  the  *ELE-
MENT_SHELL input section. 
EQ.1.0:  top surface, 
EQ.0.0:  mid-surface (default), 
EQ.-1.0:  bottom surface. 
MAREA 
Non-structural mass per unit area.  This is additional mass which
comes from materials such as carpeting.  This mass is not directly
included in the time step calculation. 
HGID 
Hourglass/bulk  viscosity  identification  defined  in  the  *HOUR-
GLASS Section: 
EQ.0: default values are used. 
ADPOPT 
Indicate  if  this  part  is  adapted  or  not.    Also  see,  *CONTROL_-
ADAPTIVITY: 
EQ.0: no adaptivity, 
EQ.1: H-adaptive for 3-D thin shells. 
THSHEL 
Thermal shell formulation 
EQ.0: Default is governed by THSHEL on *CONTROL_SHELL
EQ.1: Thick thermal shell 
EQ.2: Thin thermal shell
VARIABLE   
DESCRIPTION
TSHEAR 
Flag for transverse shear stress distribution :
FS 
FD 
DC 
VC 
EQ.0: Parabolic, 
EQ.1: Constant through thickness. 
Static coefficient of friction.  The functional coefficient is assumed
to  be  dependent  on  the  relative  velocity  vrel  of  the  surfaces  in 
contact as 
𝜇𝑐 = FD + (FS − FD)𝑒−DC×∣𝑣rel∣. 
Dynamic  coefficient  of  friction.    The  functional  coefficient  is
assumed  to  be  dependent  on  the  relative  velocity  vrel  of  the 
surfaces in contact as 
𝜇𝑐 = FD + (FS − FD)𝑒−DC×∣𝑣rel∣. 
Exponential  decay  coefficient.    The  functional  coefficient  is
assumed  to  be  dependent  on  the  relative  velocity  vrel  of  the 
surfaces in contact as 
𝜇𝑐 = FD + (FS − FD)𝑒−DC×∣𝑣rel∣. 
Coefficient  for  viscous  friction.    This  is  necessary  to  limit  the
friction  force  to  a  maximum.    A  limiting  force  is  computed
𝐹lim = VC × 𝐴cont.    Acont  being  the  area  of  the  segment  contacted 
by the node in contact.  The suggested value for VC is to use the 
  where  𝜎0    is  the  yield  stress  of  the 
yield  stress  in  shear  VC =
𝜎𝑜
√3
contacted material. 
OPTT 
Optional contact thickness.  This applies to shells only. 
SFT 
SSF 
Optional thickness scale factor for PART ID in automatic contact
(scales  true  thickness).    This  option  applies  only  to  contact  with
shell  elements.    True  thickness  is  the  element  thickness  of  the
shell elements. 
Scale  factor  on  default  slave  penalty  stiffness  for  this  PART  ID 
whenever it appears in the contact definition.  If zero, SSF is taken
as unity. 
MIDi 
Material ID of integration point I, see *MAT_… Section. 
THICKi 
Thickness of integration point i.
Bi 
*PART_COMPOSITE 
DESCRIPTION
Material angle of integration point i.  This material angle applies 
only to material types 21, 22, 23, 33, 33_96, 34, 36, 40, 41-50, 54, 55, 
58, 59, 103, 103_P, 104, 108, 116, 122, 133, 135, 135_PLC, 136, 157, 
158, 190, 219, 226, 233, 234, 235, 242, and 243. 
TMIDi 
Thermal material ID of integration point i 
PLYIDi 
Ply ID of integration point i (for post-processing purposes) 
SHRFACi 
Trnansverse shear stress scale factor 
Remarks: 
1.  Orthotropic  Materials.    In  cases  where  there  is  more  than  one  orthotropic 
material  model  referenced  by  *PART_COMPOSITE,  the  orthotropic  material 
orientation parameters (AOPT, BETA, and associated vectors) from the material 
model of the first orthotropic integration point apply to all the orthotropic inte-
gration points.  AOPT, BETA, etc.  input for materials of subsequent integration 
points is  ignored.  Bi,  not to be confused with BETA,  is taken into  account for 
each integration point. 
2.  SHRF Field and Zero Traction Condition.  Thick shell formulations 1, 2, and 
3, and all shell formulations with the exception of BCIZ and DK elements, are 
based  on  first  order  shear  deformation  theory  that  yields  constant  transverse 
shear  strains  which  violates  the  condition  of  zero  traction  on  the  top  and  bot-
tom  surfaces  of  the  shell.    For  these  elements,  setting SHRF=0.83333  will  com-
pensate for this error and result in the correct transverse shear deformation, so 
long as all layers have the same transverse stiffness.  SHRF is not used by thick 
shell forms 3, 5, or 7 except for materials 33, 36, 133, 135, and 243. 
3.  Thick Shell 5 or 6 and Shear Stress.  Thick shell formulation 5 and 6 will look 
to  the  TSHEAR  parameter  and  use  either  a  parabolic  transverse  shear  stress 
distribution  when  TSHEAR=0,  or  a  constant  shear  stress  distribution  when 
TSHEAR=1.  The parabolic option is recommended when elements are used in 
a  single  layer  to  model  a  plate  or  beam.    The  constant  option  may  be  better 
when  elements  are  stacked  so  there  are  two  or  more  elements  through  the 
thickness. 
4.  Laminated  Shear  Stress  Theory  to  Minimize  Discontinuities.    For  compo-
sites that have a transverse shear stiffness that varies by layer, laminated shell 
theory,  activated  by  LAMSHT  on  *CONTROL_SHELL,  will  correct  the  trans-
verse  shear  stress  to minimize  stress  discontinuities  between  layers  and  at  the 
bottom and top surfaces by imposing a parabolic transverse shear stress.  SHRF
should  be  set  to  the  default  value  of  1.0  when  the  shear  stress  distribution  is 
parabolic.    If  thick  shells  are  stacked  so  that  there  is  more  than  one  element 
through the thickness of a plate or beam model, setting TSHEAR=1 will cause a 
constant  shear  stress  distribution  which  may  be  more  accurate  than  parabolic.  
The  TSHEAR  parameter  is  available  for  all  thick  shell  forms  when  laminated 
shell theory is active.  Alternatively, a scale factor can be defined for transverse 
shear stress in each layer of shell or thick shell composites using the SHRFAC 
parameter.  The inputted SHRFAC values are normalized so that overall shear 
stiffness is unaffected by the distribution.  Therefore, only the ratio of parame-
ter values is significant. 
5.  Assignment  of  Zero  Thickness  to  Integration  Points.    The  ability  to  assign 
zero- thickness integration points in the stacking sequence allows the number of 
integration points to remain constant even as the number of physical plies var-
ies  from  part  to  part  and  eases  post-processing  since  a  particular  integration 
point corresponds to a physical ply.  Such a capability is important when one or 
more of the physical plies are not continuous across a composite structure.  To 
represent a missing ply in *PART_COMPOSITE, set THICKi to 0.0 for the corre-
sponding integration point and additionally, either set MID=-1 or, if the LONG 
option is used, set PLYID to any nonzero value. 
To carry this concept a step further, in cases where the number of physical plies 
varies from element to element in a  part, one can assign zero thickness to inte-
gration  points  in  exactly  the  same  manner  as  described  above  but  on  an  ele-
ment-by-element  basis  using  *ELEMENT_SHELL_COMPOSITE(_LONG)  or 
*ELMENT_TSHELL_COMPOSITE.  
When  postprocessing  the  results  using  LS-PrePost  version  4.5,  read  both  the 
keyword deck and d3plot database into the code and then select    Option > N/A 
gray  fringe.    Then,  when  viewing  fringe  plots  for  a  particular  integration  point 
(FriComp > IPt > intpt#),  the  element  will  be  grayed  out  if  the  selected  integra-
tion point is missing (or has zero thickness) in that element.
The available OPTION is 
NULL_OVERLAY 
*PART_DUPLICATE 
This option is used to generate null shells for contact. 
Purpose:  To provide a method of duplicating parts or part sets without the need to use 
the *INCLUDE_TRANSFORM option. 
Duplication  Cards.    This  format  is  used  when  the  keyword  option  is  left  <BLANK>. 
Include  as  many  of  these  cards  as  desired.   This  input  ends  at  the  next  keyword  (“*”) 
card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PTYPE 
TYPEID 
IDPOFF 
IDEOFF 
IDNOFF 
TRANID 
Type 
A 
I 
Default 
none 
none 
I 
0 
I 
0 
I 
0 
I 
0 
Null  Duplication  Cards.    This  format  is  used  when  the  keyword  option  is  set  to 
NULL_OVERLAY.  Include as many of these cards as desired.  This input ends at the 
next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
Variable 
PTYPE 
TYPEID 
IDPOFF 
IDEOFF 
DENSITY 
Type 
A 
I 
Default 
none 
none 
I 
0 
I 
0 
F 
0 
8 
6 
E 
F 
0 
7 
PR 
F 
0 
  VARIABLE   
PTYPE 
DESCRIPTION
Set to “PART” to duplicate a single part or “PSET” to duplicate a
part set. 
TYPEID 
ID of part or part set to be duplicated.
VARIABLE   
DESCRIPTION
IDPOFF 
ID offset of newly created parts. 
IDEOFF 
ID offset of newly created elements. 
IDNOFF 
ID offset of newly created nodes. 
TRANID 
ID  of  *DEFINE_TRANSFORMATION  to  transform  the  existing 
nodes in a part or part set. 
DENSITY 
Density. 
E 
PR 
Young’s modulus. 
Poisson’s ratio. 
Remarks: 
1.  All  parts  sharing  common  nodes  have  to  be  grouped  in  a  *PART_SET  and 
duplicated in a single *PART_DUPLICATE command so that the newly dupli-
cated parts still share common nodes 
2.  The following elements which need a PART to complete their definition can be 
duplicated  by  using  this  command:  *ELEMENT_SOLID,  *ELEMENT_DIS-
CRETE, *ELEMENT_SHELL, *ELEMENT_TSHELL, *ELEMET_BEAM and *EL-
EMENT_SEATBELT. 
3.  This command only duplicates definition of nodes, elements and parts, not the 
associated constraints.  For example, TC and RC defined in *NODE will not be 
passed to the newly created nodes. 
4.  When  IDNOFF = IDPOFF = IDEOFF = 0,  the  existing  part,  or  part  set,  will  be 
transformed as per TRANID, no new node or elements will be created. 
5.  The NULL_OVERLAY option may be used to generate 3 and 4-node null shell 
elements  from  the  6-  and  8-node  quadratic  elements  for  use  in  contact.    No 
additional nodes are generated.
*PART_MODES 
Purpose:    Treat  a  part  defined  with  *MAT_RIGID  as  a  linearized  flexible  body  (LFB) 
whereby  deformations  are  calculated  from  mode  shapes.    Unlike  superelements 
(*ELEMENT_DIRECT_MATRIX_INPUT),  linearized  flexible  bodies  are  accurate  for 
systems undergoing large displacements and large rotations.   
Currently,  linearized  flexible  bodies  cannot  share  nodes  with  other  linearized  flexible 
bodies or rigid bodies; however, interconnections to other linearized flexible bodies or 
to rigid bodies can use the penalty joint option.  The linearized flexible bodies are not 
implemented  with  the  Lagrange  multiplier  joint  option  . 
The deformations are modeled using the modes shapes obtained experimentally or in a 
finite element analysis, e.g., NASTRAN .pch file or a LS-DYNA d3eigv or d3mode file.  
These  files  may  contain  a  combination  of  normal  modes,  constraint  modes,  and 
attachment  modes.    For  stress  recovery  in  linearized  flexible  bodies,  use  of  linear 
element  formulations  is  recommended.    A  lump  mass  matrix  is  assumed  in  the 
implementation.  See also *CONTROL_RIGID. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
NMFB 
FORM 
ANSID 
FORMAT  KMFLAG 
NUPDF 
SIGREC 
Type 
I 
  Card 2 
1 
I 
2 
I 
3 
I 
4 
I 
5 
I 
6 
I 
7 
8 
Variable 
Type 
Default 
FILENAME 
C 
none
Kept Mode Cards.  Additional card KMFLAG = 1.  Use as many cards as necessary to 
specify  the  NMFB  kept  modes.    After  NMFB  modes  are  defined  no  further  input  is 
expected.  
  Card 3. 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MODE1  MODE2  MODE3  MODE4  MODE5  MODE6  MODE7  MODE8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
nont 
none 
nont 
none 
nont 
none 
nont 
Optional Modal Damping Cards.  This input ends at the next keyword (“*”) card. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MSTART  MSTOP 
DAMPF 
Type 
I 
I 
F 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION
PID 
Part identification.  This part must be a rigid body. 
NMFB 
Number  of  kept  modes  in  linearized  flexible  body.    The  number
of modes in the file, FILENAME, must equal or exceed NMFB.  If
KMFLAG = 0 the first NMFB modes in the file are used. 
FORM 
Linearized flexible body formulation.  See remark 5 below. 
EQ.0: exact 
EQ.1: fast 
EQ.3:  general formulation (default) 
EQ.4:  general 
formulation  without 
rigid  body  mode
orthogonalization. 
ANSID 
Attachment node set ID (optional). 
FORMAT 
Input format of modal information:
*PART_MODES 
DESCRIPTION
EQ.0: NASTRAN.pch file. 
EQ.1: (not supported) 
EQ.2: NASTRAN.pch  file  (LS-DYNA  binary  version).    The 
binary  version  of  this  file  is  automatically  created  if  a
NASTRAN.pch file is read.  The name of the binary file is
the  name  of  the  NASTRAN.pch  file  but  with  ".bin"  ap-
pended.  The binary file is smaller and can be read much
faster. 
EQ.3: LS-DYNA d3eigv binary eigenvalue database .   
EQ.4: LS-DYNA  d3mode  binary  constraint/attachment  mode
database . 
KMFLAG 
Kept  mode  flag.    Selects  method  for  identifying  modes  to  keep.
This flag is not supported for FORMAT = 4 (d3mode). 
EQ.0: the first NMFB modes in the file, FILENAME, are used. 
EQ.1: define NMFB kept modes with additional input. 
NUPDF 
Nodal  update  flag.    If  active,  an  attachment  node  set,  ANSID,
must be defined. 
EQ.0: all nodes of the rigid part are updated each cycle. 
EQ.1: only  attachment  nodes  are  fully  updated.    All  nodes  in
the  body  are  output  based  on  the  rigid  body  motion 
without  the  addition  of  the  modal  displacements.    For
maximum  benefit  an  attachment  node  set  can  also  be
defined  with  the  PART_ATTACHMENT_NODES  op-
tion.    The  same  attachment  node  set  ID  should  be  used
here.
VARIABLE   
DESCRIPTION
SIGREC 
Stress recovery flag. 
EQ.0: Do not recover stress. 
EQ.1: Recover stress. 
EQ.2: Recover  stress  and  then  set  the  recovery  stress  as  initial
stress  when  switching  to  a  deformable  body  via  *DE-
FORMABLE_TO_RIGID_AUTOMATIC.    (shell  formula-
tions 16, 18, 20, 21 and  solid formulation 2). 
EQ.3: Recover  stress  based  on  shell  formulation  21,  and  then
set  the  recovery  stress  as  initial  stress  for  shell  formula-
tion  16  when  switching  to  a  deformable  body  via  *DE-
(shell 
FORMABLE_TO_RIGID_AUTOMATIC 
formulation 16 only). 
FILENAME 
The  path  and  name  of  a  file  which  contains  the  modes  for  this
rigid body. 
MODEn 
Keep normal mode, MODEn. 
MSTART 
First mode for damping, (1 ≤ MSTART ≤ NMFB). 
MSTOP 
Last  mode  for  damping,  MSTOP,  (1 ≤ MSTOP ≤ NMFB).    All 
modes between MSTART and MSTOP inclusive are subject to the
same modal damping coefficient, DAMPF. 
DAMPF 
Modal damping coefficient, 𝜁 . 
Remarks: 
1.  The format of the file which contains the normal modes follows the file formats 
of NASTRAN output for modal information. 
2.  The  mode  set  typically  combines  both  normal  modes  and  attachment  modes.  
The eigenvalues for the attachment modes are computed from the stiffness and 
mass matrices. 
3.  The part ID specified must be either a single rigid body or a master rigid body 
  which  can  be  made  up  of  many  rigid 
parts.   
4.  The  modal  damping  is  defined  by  the  modal  damping  coefficient  𝜁 ,  where  a 
value  of  1.0  equals  critical  damping.    For  a  one  degree  of  freedom  model  sys-
tem,  the  relationship  between  the  damping  and  the  damping  coefficient  is
𝑐 = 2𝜁 𝜔𝑛𝑚,  where  c  is  the  damping,  m  is  the  mass,  and  𝜔𝑛  is  the  natural  fre-
quency, √𝑘/𝑚. 
5.  There  are  four  formulations.    The  first  is  a  formulation  that  contains  all  the 
terms of the linearized flexible body equations, and its cost grows approximate-
ly as the square of the number of modes.  The second formulation ignores most 
of  the  second  order terms  appearing  in  the  exact  equations  and  its  cost  grows 
linearly with the number of modes.  If the angular velocities are small and if the 
deflections  are  small  with  respect  to  the  geometry  of  the  system,  the  cost  sav-
ings of the second formulation may make it more attractive than the first meth-
od. 
Please note that the first two formulations are only applicable when the modes 
are eigenmodes computed for the free-free problem, that is including the 6 rigid 
body modes.  The third formulation, the default, is a more general formulation 
which allows more general mode shapes.  It is strongly recommended that the 
default formulation be used.  The fourth formulation does not orthogonalize the 
modes  with  respect  to  the  rigid  body modes,  and  may  allow  boundary  condi-
tions to be imposed more simply in some cases that the third formulation.
*PART 
Purpose:  Translate a  part by an incremental displacement in either a local or a global 
coordinate  system.    This  option  currently  applies  to  parts  defined  either  by  shell  and 
solid  elements.    All  nodal  points  of  the  given  part  ID  are  moved.    Care  must  be 
observed since parts that share boundary nodes with the part being moved must also be 
moved to avoid severe mesh distortions – the variable IFSET can be used to handle the 
situation. 
Part/Part Set Move Cards.  Include as many of following cards as desired.  This input 
ends at the next keyword (“*”) cards. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
PID/PSID 
XMOV 
YMOV 
ZMOV 
CID 
IFSET 
Type 
I 
F 
Default 
none 
0.0 
F 
0.0 
F 
0.0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
PID/PSID 
Part or part set identification number. 
XMOV 
YMOV 
ZMOV 
CID 
Move  shell/solid  part  ID,  PID,  in  the  x-direction  by  the 
incremental distance, XMOV. 
Move  shell/solid  part  ID,  PID,  in  the  y-direction  by  the 
incremental distance, YMOV. 
Move  shell/solid  part  ID,  PID,  in  the  z-direction  by  the 
incremental distance, ZMOV. 
Coordinate system ID to define incremental displacement in local
coordinate  system.    All  displacements,  XMOV,  YMOV,  and
ZMOV, are with respect to CID. 
EQ.0: global 
IFSET 
Indicate if part set ID (SID), is used in PID/SID definition. 
EQ.0: part ID (PID) is used  
EQ.1: part set ID (SID) is used.
*PART_MOVE 
1.  A new variable IFSET is added to address the move of multiple parts that share 
common boundary nodes, e.g., in case of tailor-welded blanks.  The new varia-
ble  allows  for  a  part  set  to  be  move  simultaneously.    For  example,  keyword 
*SET_PART_LIST  can  be  used  to  include  all  tailor  welded  blank  part  IDs  and 
the resulting Part Set ID can be used in this keyword. 
2.  Draw beads can be modeled as beam elements and moved in the same distance 
and direction as either the die or punch, depending on the draw types. 
3.  A partial keyword input is provided below to automatically position all tools in 
a toggle draw of a decklid inner, with a tailor welded blank consisting of PID 1 
and PID5, as shown in Figure 31-1.  With the use of the keyword *CONTROL_-
FORMING_AUTOPOSITION_PARAMETER_SET, the tailor-welded blank part 
set  ID  1  is  to  be  positioned  in  the  global  Z-direction  on  top  of  the  lower  die 
cavity (part set ID 4); the binder (part set ID 3) is to be positioned on top of the 
blank; and finally the upper punch (part set ID 2) is to be positioned on top of 
the  blank.    The  three  positioning  distances  for  the  blank,  upper  binder  and 
upper punch are calculated and stored in variables &blnkmv, &upbinmv, and 
&uppunmv,  respectively.    The  keyword  *PART_MOVE,  with  IFSET  of  “1”,  is 
responsible to actually move the three part sets, using the three corresponding 
positioning  variables.    It  is  noted  that  the  AUTOPOSITION  keyword  is  only 
applicable to shell elements. 
*PARAMETER 
R   blnkmv       0.0 
R  upbinmv       0.0 
R  uppunmv       0.0 
*SET_PART_LIST 
1 
1,5 
*SET_PART_LIST 
2 
2 
*SET_PART_LIST 
3 
3 
*SET_PART_LIST 
4 
4 
*CONTROL_FORMING_AUTOPOSITION_PARAMETER_SET 
$  PID/SID       CID       DIR MPID/MSID  Position   PREMOVE     THICK  
PARORDER 
         1                   3         4         1                 1.5    
blnkmv 
         3                   3         1         1                 1.5   
upbinmv 
         2                   3         1         1                 1.5   
uppunmv 
$---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+---
-8 
*PART_MOVE 
$    PID            XMOV            YMOV            ZMOV     CID   IFSET 
       1             0.0             0.0         &blnkmv               1
3             0.0             0.0        &upbinmv               1 
       2             0.0             0.0        &uppunmv               1 
PID 2 / PSID 2
Upper punch
PID 3 / PSID 3
Upper binder
PID 5 / PSID 1
Blank #2
Laser weld line
PID 1 / PSID 1
Blank #1
PID 4 / PSID 4
Lower cavity
  Figure 31-1.  A tailor welded blank is positioned in a decklid (toggle draw). 
Revision information: 
This  IFSET  feature  is  available  starting  in  LS-DYNA  Revision  #62935.    It  is  also 
implemented  in  all  the  applicable  stamping  processes  in  LS-PrePost4.0  Metal Forming 
Application 
eZ-Setup 
(http://ftp.lstc.com/anonymous/outgoing/lsprepost/4.0/metalforming/).
*PART_SENSOR 
Purpose:  Activate and deactivate parts, based on sensor defined in ELEMENT_SEAT-
BELT_SENSOR.  This option applies to discrete beam element only. 
Sensor Part Coupling Cards.  Include as many of the following cards as desired.  This 
input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
SIDA 
ACTIVE 
Type 
Default 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
PID 
SIDA 
ACTIVE 
Part ID, which is controlled by sensor 
Sensor ID to activate or deactivate part. 
Flag.    If  zero,  the  part  is  active  from  time  zero  until  a  signal  is
received by the part to deactivate.  If one, the part is inactive from
time  zero  and  becomes  active  when  a  signal  is  received  by  the
part  to  activate.    The  history  variables  for  inactive  parts  are 
initialized at time zero.
*PART 
Purpose:    This  keyword  provides  a  method  of  defining  a  stacked  element  model  for 
shell-like structures.  These types of plane load-bearing components possess a thickness 
which is small compared to their other (in-plane) dimensions.  Their physical properties 
vary  in  the  thickness  direction  according  to  distinct  layers.    Application  examples 
include sandwich plate systems, composite laminates, plywood, and laminated glass. 
With this keyword it is possible to discretize layered structures by an arbitrary sequence 
of  shell  and/or  solid  elements  over  the  thickness.    Whether  a  physical  ply  should  be 
discretized  by  shell  or  solid  elements  depends  on  the  individual  thickness  and  other 
mechanical  properties.    Every  single  layer  can  consist  of  one  shell  element  over  the 
thickness or one or several solid elements over thickness. 
The  stacked  element  mesh  can  either  be  provided  directly  or  it  be  automatically 
generated by LS-DYNA itself.  For automatic generation extrusion methods are used to 
determine  the  new  node  locations  that  characterize  the  out-of-plane  geometry.    Each 
layer  gets  its  own  predefined  properties  such  as  individual  thickness,  material 
characteristic, and element type. 
A  more  detailed  description  of  this  feature  including  a  detailed  description  of  the 
appropriate mesh generation procedure is given in Erhart [2015]. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
HEADING 
C 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PIDREF 
NUMLAY  ADPOPT 
Type 
I 
I 
Default 
none 
none 
I
Layer Data Cards.  The part ID, section ID, material ID, hourglass ID, thermal material 
ID,  thickness,  and  number  of  through  thickness  solid  elements  for  each  layer  i  of  a 
stacked  element  model  are  provided  below.    The  layer  data  should  be  given 
sequentially  starting  with  the  bottommost  layer.    This  card  should  be  included 
NUMLAY  times  (one  for  each  layer).    The  definitions  in  Card  3  replace  the  usual 
*PART cards. 
  Card 3 
1 
Variable 
PIDi 
2 
SIDi 
3 
4 
5 
6 
7 
8 
MIDi 
HGIDi 
TMIDi 
THKi 
NSLDi 
Type 
I 
I 
I 
Default 
none 
none 
none 
I 
0 
I 
0 
F 
I 
none 
none 
  VARIABLE   
DESCRIPTION
HEADING 
Heading for the part composition. 
PIDREF 
Part ID of reference shell element mesh. 
NUMLAY 
Number of layers. 
ADPOPT 
Indicate 
are 
*CONTROL_ADAPTIVE): 
if  parts 
EQ.0: inactive 
adapted  or  not. 
(See 
also
PIDi 
SIDi 
MIDi 
HGIDi 
TMIDi 
EQ.1: h-adaptive refinement 
Part identification. 
Section identification for layer i defined in a *SECTION keyword.
Material identification for layer i defined in a *MAT keyword. 
Hourglass  identification  for  layer  i  defined  in  a  *HOURGLASS 
keyword. 
Thermal  material  identification  for  layer  i  defined  in  a  *MAT_-
THERMAL keyword. 
THKi 
Thickness of layer i.
DESCRIPTION
Number of through-thickness solid elements for layer i. 
  VARIABLE   
NSLDi 
Remarks: 
1.  Provided  vs.    Automatically  Generated  Meshes.    In  general,  there  are  two 
different options for this keyword: 
a)  The user provides a finished mesh comprising stacked shell and/or solid 
elements  and  then  combines  the  corresponding  part  IDs  using  this  key-
word.  This mode does not require a reference mesh in the PIDREF field 
nor does it require that either the layer thickness (THKi fields) and the the 
number of through-thickness solids elements (NSLDi fields) be specfied. 
b)  The user may provide a shell reference mesh (PIDREF) together with the 
layup  sequence.    The  stacked  element  mesh  is  automatically  generated 
during  the  initialization  phase  of  LS-DYNA.    In  that  second  case,  layer 
thickness  (THKi)  and  number  of  through-thickness  solids  (NSLDi)  must 
be defined. 
2.  Shell  Solid  Overlap.    In  the  mesh  generation  case,  two  consecutive  layers 
(solid-solid or solid-shell) are firmly connected, meaning that they share nodes 
in the most obvious way possible (except they are both shell element layers, see 
Remark  3  for  that  case).    This  condition  leads  to  the  necessity  that  shell  and 
solid elements partly overlap if they follow each other in the stacking sequence.  
This  deficiency  can  be  corrected  afterwards  by  subsequent  relocation  of  the 
shell mid-surfaces via NLOC on *SECTION_SHELL (only works for first or last 
layer in this stacked element approach) or appropriate adjustment of the mate-
rial stiffness for the solid elements. 
3.  Stacked  Shells.    Starting  with  the  release  of  LS-DYNA  version  R10,  it  is 
possible to define shell element layers directly on top of each other (i.e.  without 
solid  elements  in  between).    A  potential  connection/interaction  of  such  layers 
has  to  be  declared  separately  by  additional  contact  definitions  (standard,  tied, 
or tiebreak) otherwise they are free to penetrate each other. 
4.  Chained  Calculations.    This  keyword  (*PART_STACKED_ELEMENTS)  can 
also  be  used  for  modeling  multi-stage  processes.    The  *INTERFACE_SPRING-
BACK_LSDYNA  card  can  be  used  to  save  a  final  state  including  deformed 
geometry, stresses, and strains to a dynain file.  In a subsequent calculation the 
*INCLUDE keyword can be used with that dynain to apply the layup sequence 
without regenerating the mesh.  LS-DYNA automatically detects if a reference 
shell element mesh is present or not.
5.  An Example.  An example specifying a three layer shell-solid-shell structure is 
given below: 
*PART_STACKED_ELEMENTS 
$ title 
sandwich 
$   pidref    numlay    
        11         3 
$#     pid       sid       mid      hgid      tmid       thk      nsld 
       100       200         1         1         0      0.25         0 
       101       201         2         0         0      0.60         3 
       102       200         1         1         0      0.15         0 
*SECTION_SHELL 
$      sid    elform      shrf       nip     propt   qr/irid 
       200         2     0.833       5.0       1.0       0.0 
$       t1        t2        t3        t4 
      0.25      0.25      0.25      0.25 
*SECTION_SOLID 
$      sid    elform 
       201        -1 
A  sandwich  structure  is  discretized  by  shell  elements  (SID = 200)  on  the  outer 
layers with part identifiers 100 and 102.  The interior of the “sandwich” consists 
of  three  solid  elements  (SID = 201,  NSLD = 3)  part  identifier  101.    In  this  case, 
the  reference  shell  mesh  belongs  to  part  11  (PIDREF).    The  thickness  of  each 
layer is defined by the value of the THK field, which will overwrite the thick-
ness  values  from  *SECTION_SHELL.    Related  materials  (MID,  TMID)  and 
hourglass types (HGID) are treated as usual and therefore not shown here.
*PARTICLE 
Purpose:  To define control parameters for particle based blast loading. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LAGSID  LAGSTYPE  NODID  NODTYPE
HECID 
HECTYPE 
AIRCID 
Type 
Default 
I 
0 
  Card 2 
1 
I 
0 
2 
I 
0 
3 
I 
0 
4 
I 
0 
5 
I 
0 
6 
I 
0 
7 
8 
Variable 
NPHE 
NPAIR 
IUNIT 
Type 
Default 
I 
0 
  Card 3 
1 
I 
0 
2 
I 
0 
3 
4 
5 
6 
7 
8 
Variable 
IHETYPE  DENSITY 
ENERGY  GAMMA 
COVOL 
DETO_V 
Type 
Default 
I 
0 
  Card 4 
1 
F 
0 
2 
F 
0 
3 
F 
0 
4 
F 
0 
5 
F 
0 
6 
Variable 
DETX 
DETY 
DETZ 
TDET 
BTEND 
NID 
Type 
Default 
F 
0 
F 
0 
F 
0 
F 
0 
F 
0 
I 
0 
7
Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BCX0 
BCX1 
BCY0 
BCY1 
BCZ0 
BCZ1 
Type 
Default 
F 
0 
  Card 6 
1 
F 
0 
2 
F 
0 
3 
F 
0 
4 
F 
0 
5 
F 
0 
6 
7 
8 
Variable 
IBCX0 
IBCX1 
IBCY0 
IBCY1 
IBCZ0 
IBCZ1 
BC_P 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION
LAGSID 
Structure id for  particle structure interaction 
LAGSTYPE 
Structure type 
EQ.0: Part Set 
EQ.1: Part 
NODID 
Discrete element sphere (DES) or Smooth particle hydrodynamics
(SPH) id for the interaction between particles and nodes. 
NODTYPE 
Nodal type 
EQ.0: Node Set 
EQ.1: Node 
EQ.2: Part Set 
EQ.3: Part 
HECID 
Initial container for high explosive particle
VARIABLE   
DESCRIPTION
HECTYPE 
Structure type 
EQ.0:  Part Set 
EQ.1: Part 
EQ.2: Geometry, see *DEFINE_PBLAST_GEOMETRY 
AIRCID 
Initial geometry for air particles  
EQ.0: filled air particles to entire domain defined by Card 5 
GT.0:  Reference to *DEFINE_PBLAST_AIRGEO ID 
NPHE 
Number of high explosive particles 
NPAIR 
Number of air particles 
IUNIT 
Unit System 
EQ.0: Kg-mm-ms-K 
EQ.1: SI Units 
EQ.2: Ton-mm-s-K 
EQ.3: g-cm-us-K 
EQ.4: 𝑙𝑏𝑓 ∙ 𝑠2/𝑖𝑛- 𝑖𝑛 -s-K 
IHETYPE 
High Explosive type  
EQ.1: TNT 
EQ.2: C4 
Others: Self Define 
DENSITY 
High Explosive density 
ENERGY 
High Explosive energy per unit volume 
GAMMA 
High Explosive fraction between 𝐶𝑝 and 𝐶𝑣 
COVOL 
High Explosive co-volume 
DET_V 
High Explosive detonation velocity  
DETX 
DETY 
Detonation point 𝑥 
Detonation point 𝑦
VARIABLE   
DESCRIPTION
DETZ 
TDET 
Detonation point 𝑧 
Detonation time 
BTEND 
Blast end time 
NID 
BCX0 
BCX1 
BCY0 
BCY1 
BCZ0 
BCZ1 
An optional node ID defining the position of the detonation point.
If  defined,  its  coordinates  will  overwrite  the  DETX,  DETY,  and
DETZ defined above.   
Global domain 𝑥-min 
Global domain 𝑥-max 
Global domain 𝑦-min 
Global domain 𝑦-max 
Global domain 𝑧-min 
Global domain 𝑧-max 
IBCX0 
Boundary conditions for global domain 𝑥-min 
EQ.0: Free 
EQ.1: Rigid reflecting boundary 
IBCX1 
Boundary conditions for global domain 𝑥-max 
EQ.0: Free 
EQ.1: Rigid reflecting boundary 
IBCY0 
Boundary conditions for global domain 𝑦-min 
EQ.0: Free 
EQ.1: Rigid reflecting boundary 
IBCY1 
Boundary conditions for global domain 𝑦-max 
EQ.0: Free 
EQ.1: Rigid reflecting boundary
VARIABLE   
DESCRIPTION
IBCZ0 
Boundary conditions for global domain 𝑧-min 
EQ.0: Free 
EQ.1: Rigid reflecting boundary 
IBCZ1 
Boundary conditions for global domain 𝑧-max 
EQ.0: Free 
EQ.1: Rigid reflecting boundary 
BC_P 
Pressure ambient boundary condition for global domain 
EQ.0: Off (Default) 
EQ.1: On (Remark 2) 
Remarks: 
1.  Common Material Constants for commonly used High Explosives. 
IHETYPE 
𝜌 
TNT 
1630
C4 
1601
kg
m3 
kg
m3 
𝑒0 
GJ
m3 
GJ
m3 
𝛾 
COV 
D 
1.35 
0.6 
6930
1.32 
0.6 
8193
2.  Pressure  Boundary  Conditions.    If  pressure  boundary  conditions  are  used, 
particles will  not escape from the global domain when the pressure in the do-
main is lower than the ambient.
The  keyword  *PERTURBATION  provides  a  means  of  defining  deviations  from  the 
designed structure such as buckling imperfections.  These perturbations can be viewed 
in LS-PREPOST as user-defined fringe plots.  Available options are: 
*PERTURBATION_MAT 
*PERTURBATION_NODE 
*PERTURBATION_SHELL_THICKNESS
*PERTURBATION_OPTION 
Available options are: 
MAT 
NODE 
SHELL_THICKNESS 
Purpose:  Define a perturbation (stochastic field) over the whole model or a portion of 
the  model,  typically  to  trigger  an  instability.    The  NODE  option  modifies  the  three 
dimensional  coordinates  for  the  whole  model  or  a  node  set.    For  the  SHELL_THICK-
NESS option the shell thicknesses are perturbed for the whole model or a shell set.  The 
MAT  option  perturbs  a  material  parameter  value  for  all  the  elements  associated  with 
that material. 
Material  Perturbation  Card.    Card  1  for  MAT  keyword  option.    Perturb  a  material 
parameter. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TYPE 
PID 
SCL 
CMP 
ICOORD 
CID 
Type 
Default 
I 
1 
I 
0 
F 
1.0 
I 
7 
I 
0 
I 
0 
Node Perturbation Card.  Card 1 for NODE keyword option.  Perturb the coordinates 
of a node set (or all nodes). 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TYPE 
NSID 
SCL 
CMP 
ICOORD 
CID 
Type 
Default 
I 
1 
I 
0 
F 
1.0 
I 
7 
I 
0 
I
Shell Thickness Card.  Card 1 for SHELL_THICKNESS keyword option.  Perturb the 
thickness of a set of shells (or all shells). 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TYPE 
EID 
SCL 
ICOORD 
CID 
Type 
Default 
I 
1 
I 
0 
F 
1.0 
I 
0 
I 
0 
Harmonic  Perturbation  Cards  (TYPE = 1).    Card  format  2  for  TYPE = 1.    Include  as 
many  cards  of  the  following  card  as  necessary.    The  input  ends  at  the  next  keyword 
(“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
AMPL 
XWL 
XOFF 
YWL 
YOFF 
ZWL 
ZOFF 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
1.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Fade Field Perturbation Card (TYPE = 2).  Card format 2 for TYPE = 2. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FADE 
Type 
F 
Default 
1.0
Perturbation From File Card (TYPE = 3).  Card format 2 for TYPE = 3. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FNAME 
Type 
A 
Default 
none 
Spectral Field Perturbation Card (TYPE = 4).  Card format 2 for TYPE = 4 (fade fiel).. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CSTYPE 
ELLIP1 
ELLIP2 
RND 
Type 
I 
F 
F 
Default 
none 
1.0 
1.0 
I 
0 
Spectral  Perturbation  Parameter  Cards.    Include  One,  two,  or  three  cards  of  this 
format, depending on the value of CSTYPE.  
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CFTYPE 
CFC1 
CFC2 
CFC3 
Type 
I 
F 
F 
F 
Default 
none 
1.0 
1.0 
1.0 
  VARIABLE   
DESCRIPTION
TYPE 
Type of perturbation 
EQ.1: Harmonic Field 
EQ.2: Fade out all perturbations at this node set 
EQ.3: Read perturbations from a file 
EQ.4: Spectral field
VARIABLE   
DESCRIPTION
PID 
NSID 
EID 
SCL 
CMP 
Part ID. 
Node set ID.  Specify 0 to perturb all the nodes in the model. 
Element set ID.  Specify 0 to perturb all the elements in the model.
Scale factor 
Component.    For  the  NODE  option,  these  are  given  below.    For
the MAT option, see the description of the material. 
EQ.1: 𝑥 coordinate 
EQ.2: 𝑦 coordinate 
EQ.3: 𝑧 coordinate 
EQ.4: 𝑥 and 𝑦 coordinate 
EQ.5: 𝑦 and 𝑧 coordinate 
EQ.6: 𝑧 and 𝑥 coordinate 
EQ.7: 𝑥, 𝑦, and 𝑧 coordinate 
ICOORD 
Coordinate system to use; see Remarks 7, 8 and 9 
EQ.0:  Global Cartesian 
EQ.1:  Cartesian 
EQ.2:  Cylindrical (computed and applied) 
EQ.3:  Spherical (computed and applied) 
EQ.-2:  Computed in cartesian but applied in cylindrical 
EQ.-3:  Computed in cartesian but applied in spherical 
CID 
Coordinate  system  ID,  see  *DEFINE_COORDINATE_NODES
AMPL 
Amplitude of the harmonic perturbation 
XWL 
XOFF 
YWL 
YOFF 
𝑥 wavelength of the harmonic field 
𝑥 offset of harmonic field 
𝑦 wavelength of the harmonic field 
𝑦 offset of harmonic field
VARIABLE   
DESCRIPTION
ZWL 
ZOFF 
FADE 
𝑧 wavelength of the harmonic field 
𝑧 offset of harmonic field 
Parameter  controlling  the  distance  over  which  all  *PERTURBA-
TION_NODE are faded to zero 
FNAME 
Name of file containing the perturbation definitions 
CSTYPE 
Correlation structure: 
EQ.1:  3D  isotropic.    The  𝑥,  𝑦  and  𝑧  correlations  are  described 
using one correlation function.  Define CFC1. 
EQ.2:  3D  product.    The  𝑥,  𝑦  and  𝑧  correlations  are  described 
using  a  correlation  function  each.    Define  CFC1,  CFC2
and CFC3. 
EQ.3:  2D  isotropic.    A  correlation  function  describes  the  𝑥
correlation  while  the  𝑦𝑧  isotropic  relationship  is  de-
scribed using another correlation function.  Define CFC1 
and CFC2. 
EQ.4:  2D  isotropic.    The  𝑥𝑧  isotropic  relationship  is  described 
using  a  correlation  function,  while  another  correlation
function describes the  𝑦 correlation while.  Define CFC1 
and CFC2. 
EQ.5:  2D  isotropic.    The  𝑥𝑦  isotropic  relationship  is  described 
using  a  correlation  function,  while  another  correlation
function  describes  the 𝑧  correlation  while.    Define  CFC1 
and CFC2. 
EQ.6:  3D elliptic.  Define CSE1, CSE2 and CFC1. 
EQ.7:  2D  elliptic.    A  correlation  function  describes  the  𝑥
correlation  while  the  𝑦𝑧  elliptic  relationship  is  described 
using  another  correlation  function.    Define  CSE1  and
CFC1. 
EQ.8:  2D  elliptic.    A  correlation  function  describes  the  𝑦
correlation  while  the 𝑧𝑥  elliptic  relationship  is  described 
using  another  correlation  function.    Define  CSE1  and 
CFC1. 
EQ.9:  2D elliptic.  The 𝑥𝑦 elliptic relationship is described using 
a correlation function, while another correlation function
describes  the  𝑧  correlation  while.    Define  CSE1  and
VARIABLE   
DESCRIPTION
CFC1. 
ELLIP1 
Elliptic constant for 2D and 3D elliptic fields 
ELLIP2 
Elliptic constant for 3D elliptic field 
RND 
Seed for random number generator. 
EQ.0: LS-DYNA will generate a random seed 
GT.0:  Value to be used as seed 
CFTYPE 
Correlation function 
EQ.1: Gaussian 
EQ.2: Exponential 
EQ.3: Exponential Cosine 
EQ.4: Rational 
EQ.5: Linear 
CFCi 
Correlation function constant i 
Remarks: 
1.  Postprocessing.  The  perturbation  can  be  viewed  in  LS-PrePost.    For  the 
NODE  option,  LS-DYNA  creates  files  named pert_node_x/y/z/res,  which 
can  be  viewed  as  user-defined  fringe  plots.    For  the  SHELL_THICKNESS  and 
MAT  options,  the  files  are  named  pert_shell_thickness  and  pert_mat 
respectively.  If a coordinate system with a radial component is used, then the 
file pert_node_radial is also written. 
2.  Linear  Combinations  and  Maximum  Amplitudes.    Perturbations  specified 
using separate *PERTURBATION cards are created separately and then added 
together.    This  is  true  as  well  for  special  cases  such  as  CMP = 7  in  which  case 
the  𝑥,  𝑦  and  𝑧  fields  are  created  separately  and  added  together  afterwards, 
which  can  result  in  an  absolute  amplitude  greater  than  specified  using  AMPL 
or SCL. 
3.  Harmonic Perturbations.  The harmonic perturbation is
𝑝CMP(𝑥, 𝑦, 𝑧) = SCL
× AMPL× [sin (2𝜋
𝑥 + XOFF
XWL
) + sin (2𝜋
𝑦 + YOFF
YWL
)
+ sin (2𝜋
𝑧 + ZOFF
ZWL
)] 
Note  that  the  harmonic  perturbations  can  sum  to  values  greater  than  SCL × 
AMPL. 
4.  The Fade Perturbation.  The fade perturbation is 
𝑝′(𝑥, 𝑦, 𝑧) = 𝑆𝐶𝐿 × (1 −
𝑒FADE×𝑥′) 𝑝(𝑥, 𝑦, 𝑧) 
where 𝑥′ the shortest distance to a node in the node set specified and FADE the 
parameter controlling the sharpness of the fade perturbation. 
5.  Keyword  Format  for  FNAME  Field.    The  file  FNAME  must  contain  the 
perturbation  in  the  LS-DYNA  keyword  format.    This  file  can  be  created  from 
the  d3plot  results  using  the  LS-PrePost  Output  capability.    The  data  must  be 
arranged  into  two  columns  with  the  first  column  being  the  node  ids.    Lines 
starting with the character $ will be ignored. 
6.  Correlation Functions.  The correlation functions are defined as follows: 
a)  Gaussian: 𝐵(𝑡) = 𝑒−(𝑎𝑡)2
b)  Exponential: 𝐵(𝑡) = 𝑒−|𝑎𝑡|𝑏
c)  Exponent and Cosine: 𝐵(𝑡) = 𝑒−|𝑎𝑡|cos(𝑏𝑡) 
d)  Rational: 𝐵(𝑡) = (1 + |𝑎𝑡|𝑏)−𝑐 
e)  Piecewise Linear: 𝐵(𝑡) = (1 − |𝑎𝑡|)𝜒(1 − |𝑎𝑡|) 
f)  With 𝜒 the Heaviside step function and a, b and c corresponding to CFC1, 
CFC2 and CFC3. 
7.  Cylindrical  Coordinates.    For  the  cylindrical  coordinate  system  option 
(ICOORD = 2), the default is to use the global coordinate system for the location 
of  the  cylindrical  part,  with  the  base  of  the  cylinder  located  at  the  origin,  and 
the global 𝑧-axis aligned with the cylinder axis.  For cylindrical parts not located 
at  the  global  origin,  define  a  coordinate  system  (numbered  CID)  using  *DE-
FINE_COORDINATE_NODES by selecting any three nodes on the base of the 
cylinder in a clockwise direction (resulting in the local 𝑧-axis to be aligned with 
the cylinder).
8.  Spherical  Coordinates.    For  the  spherical  coordinate  system  (ICOORD = 3), 
the  coordinates  are  the  radius,  zenith  angle [0, 𝜋],  and  the  azimuth  an-
gle [0,2𝜋].    The  default  is  to  use  the  global  coordinate  system  with  the  zenith 
measured from the 𝑧-axis and the azimuth measured from the 𝑥-axis in the 𝑥𝑦-
plane.  For spherical parts not located at the global origin, define a coordinate 
system  using  *DEFINE_COORDINATE_NODES  by  selecting  any  three  nodes 
as follows: the first node is the center of the sphere, the second specifies the 𝑥-
axis of the coordinate system, while the third point specifies the plane contain-
ing the new 𝑦-axis.  The 𝑧-axis will be normal to this plane. 
9.  Computed In Cartesian Applied to Cylindrical or Spherical.  It is possible to 
compute the perturbations in a Cartesian coordinate system, but to apply them 
in  a  cylindrical  or  spherical  coordinate  system  (ICOORD = -2, -3).    This  is  the 
natural method of doing say a radial perturbation of a sphere using a spectral 
perturbation field.  We expect that computing the perturbation in the spherical 
coordinate system should be rare (ICOORD = 3).  Computing a perturbation in 
a cylindrical coordinate system should be common though; for example, a cir-
cumferential harmonic perturbation. 
10.  Material Perturbation Feature.  Only *MAT_238 (*MAT_PERT_PIECEWISE_-
LINEAR_PLASTICITY)  and  solid  elements  in  an  explicit  analysis  can  be  per-
turbed using *PERTURBATION_MAT.  See the documentation of this material 
for  allowable  components.    Only  one  part  per  model  can  be  perturbed.    For 
some perturbed quantity c, the material perturbation is applied on an element-
by-element basis as 
𝑐new = (1 + 𝑝)𝑐base 
where 𝑝 is a random number, which is written to the pert_mat file during the 
calculation.  Values of 𝑝 less than -1 are not allowed because the material behav-
ior is not defined.   
Completely independent of *PERTURBATION_MAT, see *DEFINE_STOCHAS-
TIC_VARIATION  for  a  way  to  define  a  stochastic  variation  of  yield  stress 
and/or  failure  strain  in  material  models  10,  15,  24,  81,  and  98  and  the  shell 
version of material 123. 
.
Two keywords are defined in this section. 
*RAIL_TRACK 
*RAIL_TRAIN
*RAIL_TRACK 
Purpose:  Wheel-rail contact algorithm intended for railway applications but can also be 
used  for  other  purposes.    The  wheel  nodes  (defined  on  *RAIL_TRAIN)  represent  the 
contact patch between wheel and rail.  A penalty method is used to constrain the wheel 
nodes to slide along the track.  A track consists of two rails, each of which is defined by 
a set of beam elements. 
Card Sets.  For each track include one pair of cards 1 and 2.  This input ends at the next 
keyword (“*”) card. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
BSETID1  NORGN1 
LCUR1 
OSET1 
SF1 
GA1 
IDIR 
Type 
I 
I 
I 
I 
F 
F 
F 
Default 
none 
none 
none 
none 
0.0 
1.0 
0.0 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
Variable 
blank 
BSETID2  NORGN2 
LCUR2 
OSET2 
SF2 
GA2 
Type 
Default 
- 
- 
I 
I 
I 
F 
F 
F 
none 
none 
none 
0.0 
1.0 
0.0 
I 
0 
8 
  VARIABLE   
DESCRIPTION
ID 
Track ID 
BSETID1,2 
Beam  set  ID  for  rails  1  and  2  containing  all  beam  elements  that
make up the rail, see *SET_BEAM. 
NORGN1,2 
Reference  node  at  one  end  of  each  rail,  used  as  the  origin  for  the
roughness  curve.    The  train  will  move  in  a  direction  away  from
this node.
LCUR1,2 
*RAIL 
DESCRIPTION
Load  curve  ID    defining  track  roughness 
(vertical displacement from line of beam elements) of the rail as a 
function of distance from the reference node NORIGIN.  Distance 
from  reference  node  on  x-axis  of  curve,  roughness  on  y-axis. 
Default: no roughness. 
OSET1,2 
Origin  of  curve  LCUR  is  shifted  by  distance  OSET  towards  the
reference node. 
SF1,2 
GA1,2 
IDIR 
Roughness values are scaled by SF.  Default: 1.0. 
Shear  stiffness  of  rail  per  unit  length  (used  to  calculate  local  rail
  GA = shear 
shear  deformation  within  each  beam  element). 
modulus x cross-sectional area.  Default: local shear deformation is 
ignored. 
Determines which way is “up” for purposes of wheel/rail contact.
Vertical  contact  works  like  a  normal  penalty-based  contact  while 
horizontal contact follows Figure 34-2. 
EQ.0:  (Default)    global  z  is  “up”  and  the  global  x-y  plane  is 
assumed  horizontal  irrespective  of  the  geometry  of  the
rails. 
EQ.1:  “Up”  is  the  normal  vector  to  the  plane  containing  the  2
rails, given by the vector c where c = (a x b), a is the direc-
tion along rail 1 heading away from node NORGN1 and 
b is the vector from rail 1 to rail 2.  Both a and b are de-
termined locally at the contact point 
EQ.-1:  Same as IDIR = 1 except “up” is along -c. 
Remarks: 
*RAIL_TRACK  and  *RAIL_TRAIN  were  written  by  Arup  to  represent  wheel-rail 
contact.    They  have  been  used  to  generate  loading  on  models  of  bridges  for  vibration 
predictions,  stress  calculations  and  for  estimating  accelerations  experienced  by 
passengers.    Other  non-railway  uses  are  possible:  the  algorithm  causes  the  “train” 
nodes  to  follow  the  line  defined  by  the  “rail”  beam  elements  and  transfers  forces 
between them.  In some cases (especially vibration modeling), double precision versions 
of LS-DYNA may give superior results because of the small relative deflections between 
wheel and rail.
Theoretical curve
Rail Node
Beam element
Roughness
+
=
Distance
Theoretical curve
Surface profile =
                theoretical curve + roughness
D= Distance of train node
             below surface profile
Train node
Force = VERTSTF × D
Figure 34-1.  Track Model 
Track modeling: 
The  rails  of  the  track  should  be  modeled  by two  parallel  lines  of  beam  elements.    The 
track can be curved or straight and the rails can be modeled as deformable or rigid.  If 
required,  rail  pads,  sleepers  and  ballast  may  also  be  modeled  –  typically  with  spring, 
damper  and  beam  elements.    It  is  also  possible  to  use  this  algorithm  to  control  the 
motion of simple road vehicle models: beam element “rails” made of null material can 
be embedded in the road surface.  It is recommended that the mesh size of the two rails 
should  be  similar:  LS-DYNA  calculates  a  local  coordinate  system  for  each  train  node 
based on the alignment of the currently contacted beam element and the nearest node 
on the other rail. 
Because wheel-rail contact stiffness is generally very high, and wheel masses are large, 
small deviations from a straight line or smooth curve can lead to large transient forces.  
It is recommended that great care be taken in generating and checking the geometry for
the  track,  especially  where  the  track  is  curved.    Some  pre-processors  write  the 
coordinates  with  insufficient  precision  to  the  LS-DYNA  input  file,  and  this  can  cause 
unintended  roughness  in  the  geometry.    For  the  same  reason,  if  the  line  of  the  track 
were  taken  as  straight  between  nodes,  spurious  forces  would  be  generated  when  the 
wheel  passes  from  one  rail  element  to  the  next.    This  is  avoided  because  the  *RAIL 
algorithm  calculates  a  theoretical  curved  centerline  for  the  rail  element  to  achieve 
continuity of slope from one element to the next.  Where the length of the rail elements 
is similar to or shorter than the maximum section dimension, shear deformation may be 
significant  and  it  is  possible  to  include  this  in  the  theoretical  centerline  calculation  to 
further reduce spurious forces at the element boundaries (inputs GA1, GA2). 
Roughness  (small  deviations  in  the  vertical  profile  from  a  perfect  straight  line)  does 
exist in real life and is a principal source of vibration.  *RAIL allows the roughness to be 
modeled by a load curve giving the vertical deviation (in length units) of the rail surface 
from the theoretical centerline of the beam elements as a function of distance along the 
track  from  the  origin  node  of  the  rail.    The  roughness  curve  is  optional.    Ideally, 
roughness profiles measured from both rails of the same piece of track should be used 
so that the relationship between bump and roll modes is correctly captured. 
Whether  roughness  is  included  or  not,  it  is  important  to  select  as  the  origin  nodes 
(NORIGIN1  and  NORIGIN2)  the  nodes  at  the  end  of  the  rails  away  from  which  the 
train will be traveling.  The train can start at any point along the rails but  must travel 
away from the origin nodes. 
Train modeling: 
The vehicle models are typically modeled using spring, damper and rigid elements, or 
simply a point mass at each wheel position.  Each node in the set referred to on *RAIL_-
TRAIN  represents  the  contact  patch  of  one  wheel  (note:  not  the  center  of  the  wheel).  
These nodes should be initially on or near the line defined by either of the two rails.  LS-
DYNA  will  move  the  train  nodes  initially  onto  the  rails  to  achieve  the  correct  initial 
wheel-rail  forces.    If  the  results  are  viewed  with  magnified  displacements,  the  initial 
movements can appear surprising. 
Wheel roughness input is available.  This will be applied in addition to track roughness.  
The input curve must continue for the total rolled distance – it is not assumed to repeat 
with each wheel rotation.  This is to avoid problems associated with ensuring continuity 
between  the  start  and  end  of  the  profile  around  the  wheel  circumference,  especially 
since the profiles might be generated from roughness spectra rather than taken directly 
from measured data.
Lateral
Force
Force on
Wheel B
L3
L2
Deflection
L2
L3
Force on
Wheel A
L2
L2
Figure  34-2.    Illustration  of  lateral  drift  parameters  L2  and  L3  from  *RAIL_-
TRACK. 
Wheel-rail interface: 
The wheel-rail interface model is a simple penalty function designed to ensure that the 
train nodes follow the line of the track.  It does not attempt to account for the shape of 
the rail profile.  Vertical and lateral loads are treated independently.  For this reason, the 
algorithm is not suitable for rail vehicle dynamics calculations. 
Wheel-rail contact stiffness is input on *RAIL_TRAIN.  For vertical loads, a linear force-
deflection  relationship  is  assumed  in  compression;  no  tensile  force  is  generated  (this 
corresponds  to  the  train  losing  contact  with  the  rail).    Typical  contact  stiffness  is 
2MN/mm.  Lateral deflections away from the theoretical centerline of the rail beams are 
also penalized by a linear force-deflection relationship.  The lateral force is applied only 
to  wheels  on  the  side  towards  which  the  train  has  displaced  (corresponding  to  wheel 
flanges that run inside the rails). 
Optionally,  a  “gap”  can  be  defined  in  input  parameter  L2  such  that  the  wheel  set  can 
drift laterally by L2 length units before any lateral force is generated.  A further option 
is  to  allow  smooth  transition  between  “gap”  and  “contact”  by  means  of  a  transition 
distance input as parameter L3.  Figure 34-2 illustrates the geometry of parameters L2 
and L3. 
Generally, with straight tracks a simple linear stiffness is sufficient.  With curved tracks, 
a  reasonable  gap  and  transition  distance  should  be  defined  to  avoid  unrealistic  forces 
being  generated  in  response  to  small  inaccuracies  in  the  distance  between  the  rails.  
Gravity loading is expected, in order to maintain contact between rail and wheel.  This 
is  normally  applied  by  an  initial  phase  of  dynamic  relaxation.    To  help  achieve 
convergence quickly, or in some cases avoid the need for dynamic relaxation altogether,
the initial force expected on each train node can be input (parameter FINIT on *RAIL_-
TRAIN).  LS-DYNA positions the nodes initially such that the vertical contact force will 
be  FINIT  at  each  node.    If  the  suspension  of  the  rail  vehicles  is  modeled,  it  is 
recommended that the input includes carefully calculated precompression of the spring 
elements; if this is not done, achieving initial equilibrium under gravity loading can be 
very time consuming. 
The  *RAIL  algorithm  ensures  that  the  train  follows  the  rails,  but  does  not  provide 
forward motion.  This is generally applied using *INITIAL_VELOCITY, or for straight 
tracks, *BOUNDARY_PRESCRIBED_MOTION. 
Output: 
LS-DYNA generates an additional ASCII output file train_force_n, where n is an integer 
updated  to  avoid  overwriting  any  existing  files.    The  file  contains  the  forces  on  each 
train  node,  output  at  the  same  time  intervals  as  the  binary  time  history  file  (DT  on 
*DATABASE_BINARY_D3THDT). 
Checking: 
It  is  recommended  that  track  and  train  models  be  tested  separately  before  adding  the 
*RAIL  cards.    Check  that  the  models  respond  stably  to  impulse  forces  and  that  they 
achieve  equilibrium  under  gravity  loading.    The  majority  of  problems  we  have 
encountered have been due to unstable behavior of train or track.  Often, these are first 
detected by the *RAIL algorithm and an error message will result.
*RAIL_TRAIN 
Purpose:  Define train properties.  A train is defined by a set of nodes in contact with a 
rail defined by *RAIL_TRACK. 
Card Sets.  For each train include one pair of cards 1 and 2.  This input ends at the next 
keyword (“*”) card. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
NSETID 
(omit) 
FINIT 
(omit) 
TRID 
LCUR 
OFFS 
Type 
I 
I 
F 
F 
F 
Default 
none 
none 
0.0 
0.0 
0.0 
  Card 2 
1 
2 
Variable 
VERTSTF 
LATSTF 
Type 
F 
F 
3 
V2 
F 
4 
V3 
F 
5 
L2 
F 
I 
F 
none 
0.0 
7 
8 
I 
0 
6 
L3 
F 
Default 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  VARIABLE   
DESCRIPTION
ID 
Train ID 
NSETID 
Node set ID containing all nodes that are in contact with rails. 
(omit) 
FINIT 
(omit) 
TRID 
Unused variable – leave blank. 
Estimate of initial vertical force on each wheel (optional) – speeds 
up the process of initial settling down under gravity loading. 
Unused variable – leave blank. 
ID of track for this train, see *RAIL_TRACK.
LCUR 
*RAIL 
DESCRIPTION
ID 
Load  curve 
  containing  wheel 
roughness (distance of wheel surface away from perfect circle) vs.
distance traveled.  The curve does not repeat with each rotation of
the wheel – the last point should be at a greater distance than the 
train is expected to travel.  Default: no wheel roughness. 
OFFS 
Offset  distance  used  to  generate  different  roughness  curves  for
each wheel from the roughness curve LCUR.  The curve is offset
on  the  x-axis  by  a  different  whole  number  multiple  of  OFFS  for 
each wheel. 
VERTSTF 
Vertical stiffness of rail contact. 
LATSTF 
Lateral stiffness of rail contact. 
V2,V3 
Unused variables – leave blank. 
L2 
L3 
Lateral clearance from rail to wheel rim.  Lateral force is applied
to a wheel only when it has moved more than L2 away from the 
other  rail,  i.e.    the  wheel  rims  are  assumed  to  be  near  the  inner
face of the rail. 
Further lateral distance before full lateral stiffness applies  (force-
deflection curve follows a parabola up to this point).
Two keywords are used in this section to define rigid surfaces: 
*RIGIDWALL_GEOMETRIC_OPTION_{OPTION}_{OPTION}}_{OPTION} 
*RIGIDWALL_PLANAR_{OPTION}_{OPTION}_{OPTION} 
The  RIGIDWALL  option  provides  a  simple  way  of  treating  contact  between  a  rigid 
surface and nodal points of a deformable body, called slave nodes.  Slave nodes which 
belong  to  rigid  parts  are  not,  in  general,  checked  for  contact  with  only  one  exception.  
The RIGIDWALL_PLANAR option may be used with nodal points of rigid bodies if the 
planar wall defined by this option is fixed in space and the RWPNAL parameter is set 
to a positive nonzero value on the control card, *CONTROL_CONTACT. 
When  the  rigid  wall  defined  in  this  section  moves  with  a  prescribed  motion,  the 
equations of rigid body mechanics are not involved.  For a general rigid body treatment 
with  arbitrary  surfaces  and  motion,  refer  to  the  *CONTACT_ENTITY  definition.    The 
*CONTACT_ENTITY  option  is  for  treating  contact  between  rigid  and  deformable 
surfaces only. 
Energy  dissipated  due  to  rigidwalls  (sometimes  called  stonewall  energy  or  rigidwall 
energy) is computed only if the parameter RWEN is set to 2 in *CONTROL_ENERGY.
*RIGIDWALL_FORCE_TRANSDUCER 
Purpose:    Define  a  force  transducer  for  a  rigid  wall.    The  output  of  the  transducer  is 
written to the rwforc file. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TID 
RWID 
Type 
I 
I 
Default 
none 
none 
. 
  VARIABLE   
DESCRIPTION
TID 
Transducer ID. 
RWID 
Rigid wall ID. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
Remarks 
HEADING 
C 
none
Node Set Cards.  For each node set add one card.  This input ends at the next keyword 
(“*”). 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSID 
Type 
I 
Default 
0. 
. 
Remarks 
  VARIABLE   
DESCRIPTION
NSID 
Node set ID.  
Remarks: 
1.  The forces acting on rigid wall RWID are reported separately for each NSID. 
2.  For rigid walls using the segment option, the forces acting on each segment are 
reported separately for each NSID.
*RIGIDWALL_GEOMETRIC_OPTION_{OPTION}_{OPTION}_{OPTION} 
Available options include: 
FLAT 
PRISM 
CYLINDER 
SPHERE 
If prescribed motion is desired an additional option is available: 
MOTION 
One  of  the  shape  types  [FLAT,  PRISM,  CYLINDER,  SPHERE]  must  be  specified, 
followed by the optional definition of MOTION, both on the same line with  *RIGID-
WALL_GEOMETRIC.  If an ID number is specified the additional option is available: 
ID 
If active, the ID card is the first card following the keyword.  To view the rigid wall, the 
option: 
DISPLAY 
is available.  With this option a rigid body is automatically defined which represents the 
shape,  the  physical  position  of  the  wall, and  follows  the  walls  motion  if  the  MOTION 
option is active.  Additional input is optional if DISPLAY is active. 
For the CYLINDER and SPHERE, the option: 
INTERIOR 
is available.  Nodes are confined to the interior of these geometric forms. 
Purpose:    Define  a  rigid  wall  with  an  analytically  described  form.    Four  forms  are 
possible.    A  prescribed  motion  is  optional.    For  general  rigid  bodies  with  arbitrary 
surfaces  and  motion,  refer  to  the  *CONTACT_ENTITY  definition.    This  option  is  for 
treating contact between rigid and deformable surfaces only. 
Card Sets.  For each rigid wall matching the specified keyword options include one set 
of the following data cards.  This input ends at the next keyword (“*”) card.
ID Card.  Additional card for ID keyword option. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RWID 
Type 
I 
HEADING 
A70 
This  heading  is  picked  up  by  some  of  the  peripheral  LS-DYNA  codes  to  aid  in  post-
processing.  
  VARIABLE   
DESCRIPTION
RWID 
Rigid wall ID.  This must be a unique number. 
HEADING 
Rigid wall descriptor.  It is suggested that unique descriptions be
used. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSID 
NSIDEX 
BOXID 
BIRTH 
DEATH 
Type 
I 
Default 
none 
I 
0 
I 
0 
F 
F 
0. 
1.0E+20
  VARIABLE   
DESCRIPTION
NSID 
Nodal set ID containing slave nodes, see *SET_NODE_OPTION: 
EQ.0: all nodes are slave to rigid wall. 
NSIDEX 
BOXID 
BIRTH 
Nodal set ID containing nodes that exempted as slave nodes, see
*SET_NODE_OPTION. 
If defined, only nodes in box are included as slave nodes to rigid
wall. 
Birth  time of  rigid  wall.    The  time  values  of the  load  curves  that
control the motion of the wall are offset by the birth time.
DESCRIPTION
Death time of rigid wall.  At this time the wall is deleted from the
calculation.  If dynamic relaxation is active at the beginning of the 
calculation  and  if  BIRTH = 0.0,  the  death  time  is  ignored  during 
the dynamic relaxation. 
2 
YT 
F 
0. 
3 
ZT 
F 
0. 
4 
XH 
F 
0. 
5 
YH 
F 
0. 
6 
ZH 
F 
0. 
7 
8 
FRIC 
F 
0. 
  VARIABLE   
DEATH 
  Card 3 
Variable 
1 
XT 
Type 
F 
Default 
0. 
Remarks 
  VARIABLE   
DESCRIPTION
XT 
YT 
ZT 
XH 
YH 
ZH 
𝑥-coordinate  of  tail  of  any  outward  drawn  normal  vector,  𝐧, 
originating  on  wall  (tail)  and  terminating  in  space  (head),  see
Figure 35-1. 
𝑦-coordinate of tail of normal vector 𝐧 
𝑧-coordinate of tail of normal vector 𝐧 
𝑥-coordinate of head of normal vector 𝐧 
𝑦-coordinate of head of normal vector 𝐧 
𝑧-coordinate of head of normal vector 𝐧 
FRIC 
Coulomb friction coefficient except as noted below. 
EQ.0.0: frictionless sliding after contact, 
EQ.1.0: stick condition after contact.
rectangular prism
cylinder
flat surface
sphere
Figure  35-1.    Vector  𝐧  determines  the  orientation  of  the  rigidwall.    By
including  the  MOTION  option,  motion  of  the  rigidwall  can  be  prescribed  in
any direction 𝐕 as defined by variables VX, VY, VZ. 
Flat Rigidwall Card.   Card 4 for FLAT keyword option.  A plane with a finite size or 
with an infinite size can be defined, see Figure 35-1.  The vector m is computed as the 
vector cross product 𝐧 × 𝐥.  The origin, which is the tail (the start) of the normal vector, 
is the corner point of the finite size plane.  
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
XHEV 
YHEV 
ZHEV 
LENL 
LENM 
Type 
F 
Default 
0. 
F 
0. 
F 
F 
F 
0. 
infinity 
infinity
VARIABLE   
DESCRIPTION
XHEV 
YHEV 
ZHEV 
LENL 
𝑥-coordinate of head of edge vector 𝐥, see Figure 35-1. 
𝑦-coordinate of head of edge vector 𝐥 
𝑧-coordinate of head of edge vector 𝐥 
Length of 𝐥 edge.  A zero value defines an infinite size plane. 
LENM 
Length of 𝐦 edge.  A zero value defines an infinite size plane. 
Prismatic Rigidwall Card.  Card 4 for PRISM keyword option.  The description of the 
definition of a plane with finite size is enhanced by an additional length in the direction 
negative to 𝐧, see Figure 35-1.  
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
XHEV 
YHEV 
ZHEV 
LENL 
LENM 
LENP 
Type 
F 
F 
F 
F 
F 
F 
Default 
none 
0. 
0. 
infinity 
infinity 
infinity 
  VARIABLE   
DESCRIPTION
XHEV 
YHEV 
ZHEV 
LENL 
LENM 
LENP 
𝑥-coordinate of head of edge vector 𝐥, see Figure 35-1. 
𝑦-coordinate of head of edge vector 𝐥 
𝑧-coordinate of head of edge vector 𝐥 
Length of 𝐥 edge.  A zero value defines an infinite size plane. 
Length of 𝐦 edge.  A zero value defines an infinite size plane. 
Length of prism in the direction negative to 𝐧, see Figure 35-1.
Cylinderical  Rigidwall  Card.    Card  4  for  CYLINDER  keyword  option.    The  tail  of  𝐧
specifies the top plane of the cylinder.  The length is defined in the direction negative to 
𝐧.  See Figure 35-1.  
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RADCYL 
LENCYL 
NSEGS 
Type 
F 
F 
I 
Default 
none 
infinity 
none 
  VARIABLE   
DESCRIPTION
RADCYL 
Radius of cylinder 
LENCYL 
Length  of  cylinder,  see  Figure  35-1.    Only  if  a  value  larger  than 
zero is specified is a finite length assumed. 
NSEGS 
Number of subsections 
NSEGS Card.  Additional card for NSEGS option. 
  Card 5 
Variable 
1 
VL 
2 
3 
4 
5 
6 
7 
8 
HEIGHT 
Type 
F 
F 
Default 
none 
none 
  VARIABLE   
DESCRIPTION
VL 
Distance from the Cylinder base 
HEIGHT 
Section height
Spherical  Rigidwall  Card.    Card  4  for  SPHERE  keyword  option.    The  center  of  the 
sphere is identical to the tail (start) of 𝐧, see Figure 35-1.  
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RADSPH 
Type 
F 
Default 
0. 
  VARIABLE   
DESCRIPTION
RADSPH 
Radius of sphere 
Motion Card.  Additional card for motion keyword option. 
  Card 5 
1 
2 
Variable 
LCID 
OPT 
Type 
I 
I 
3 
VX 
F 
4 
VY 
F 
5 
VZ 
F 
Default 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
6 
7 
8 
LCID 
OPT 
VX 
VY 
VZ 
Rigidwall motion curve number, see *DEFINE_CURVE. 
Type of motion: 
EQ.0: velocity specified, 
EQ.1: displacement specified. 
𝑥-direction cosine of velocity/displacement vector   
𝑦-direction cosine of velocity/displacement vector   
𝑧-direction cosine of velocity/displacement vector
Display  Card.    Optional  card  for  DISPLAY  keyword  option.    If  this  card  is  omitted 
default values are set.  The values set here have no effect on the solution other than the 
PID appearing in the postprocessing.  
5 
6 
7 
8 
  Card 6 
1 
Variable 
PID 
Type 
I 
2 
RO 
I 
3 
E 
I 
4 
PR 
F 
Default 
none 
1.0E-09  1.0E-04
0.3 
  VARIABLE   
DESCRIPTION
PID 
RO 
E 
PR 
Unique part ID for moving geometric rigid wall.  If zero, a part ID
will  be  set  that  is  larger  than  the  maximum  of  all  user  defined
part ID’s. 
Density of rigid wall.  The default is set to 1.0E-09. 
Young’s modulus.  The default is set to 1.0E-04. 
Poisson’s ratio.  The default is set to 0.30. 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *RIGIDWALL_GEOMETRIC_SPHERE_MOTION 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Define a rigid sphere: 
$     - with a radius of 8 
$     - centered at (x,y,z) = (20,20,9) 
$     - that moves in the negative z-direction with a specified displacement 
$          given by a load curve (load curve: lcid = 5) 
$     - which prevents all nodes within a specified box from penetrating the 
$          sphere (box number: boxid = 3), these nodes can slide on the sphere 
$          without friction 
$ 
*RIGIDWALL_GEOMETRIC_SPHERE_MOTION 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$     nsid    nsidex     boxid 
                             3 
$ 
$       xt        yt        zt        xh        yh        zh      fric 
      20.0      20.0       9.0      20.0      20.0       0.0       0.0 
$ 
$   radsph 
       8.0 
$ 
$     lcid       opt        vx        vy        vz 
         5         1       0.0       0.0      -1.0
$ 
$ 
*DEFINE_BOX 
$    boxid       xmn       xmx       ymn       ymx       zmn       zmx 
         3       0.0      40.0       0.0      40.0      -1.0       1.0 
$ 
$ 
*DEFINE_CURVE 
$     lcid      sidr      scla      sclo      offa      offo 
         5 
$           abscissa            ordinate 
                 0.0                 0.0 
              0.0005                15.0 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
*RIGIDWALL_PLANAR_{OPTION}_{OPTION}_{OPTION} 
Available options include: 
<BLANK> 
ORTHO 
FINITE 
MOVING 
FORCES 
The ordering of the options in the input below must be observed but the ordering of the 
options on the command line is unimportant, i.e.; the ORTHO card is first, the FINITE 
definition  card  below  must  precede  the  MOVING  definition  card,  and  the  FORCES 
definition  card  should  be  last.    The  ORTHO  option  does  not  apply  if  the  MOVING 
option is used.   
An ID number may be assigned to the rigid wall using the following option: 
ID 
If this option is active, the ID card is the first card following the keyword.   
Display  of  a  non-moving,  planar  rigid  wall  is  on  by  default  .  The option 
DISPLAY 
is  available  for  display  of  moving rigid  walls.    With  this  option  active,  a rigid  body  is 
automatically  created  which  represents  the  shape  of  the  rigid  wall  and  tracks  its 
position  without  need  for  additional  input.    The  part  ID  of  the  rigid  body  defaults  to 
RWID if the ID option is active, and if RWID is a unique ID within the set of all part IDs. 
Purpose:    Define  planar  rigid  walls  with  either  finite  (FINITE)  or  infinite  size.  
Orthotropic friction can be defined (ORTHO).  Also, the plane can possess a mass and 
an  initial  velocity  (MOVING);  otherwise,  the  wall  is  assumed  to  be  stationary.    The 
FORCES  option  allows  the  specification  of  segments  on  the  rigid  walls  on  which  the 
contact forces are computed.  In order to achieve a more physical reaction related to the 
force versus time curve, the SOFT value on the FORCES card can be specified. 
Card Sets.  For each rigid wall matching the specified keyword options include one set 
of the following data cards.  This input ends at the next keyword (“*”) card.
ID.  Card.  Additional card for ID keyword option. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RWID 
Type 
I 
Default 
none 
  VARIABLE   
DESCRIPTION
RWID 
Rigid wall ID.  Up to 8 characters can be used. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSID 
NSIDEX 
BOXID 
OFFSET 
BIRTH 
DEATH 
RWKSF 
Type 
I 
Default 
none 
I 
0 
I 
0 
F 
0. 
F 
F 
F 
0. 
1.0E+20 
1.0 
  VARIABLE   
DESCRIPTION
NSID 
Nodal set ID containing slave nodes, see *SET_NODE_OPTION: 
EQ.0: all nodes are slave to rigid wall. 
NSIDEX 
BOXID 
OFFSET 
Nodal set ID containing nodes that exempted as slave nodes, see
*SET_NODE_OPTION. 
All  nodes  in  box  are  included  as  slave  nodes  to  rigid  wall,  see
*DEFINE_BOX.  If options NSID or NSIDEX are active then only 
the subset of nodes activated by these options are checked to see 
if they are within the box. 
All  nodes  within  a  normal  offset  distance,  OFFSET,  to  the  rigid
wall  are  included  as  slave  nodes  for  the  rigid  wall.    If  options
NSID, NSIDEX, or BOXID are active then only the subset of nodes
activated by these options are checked to see if they are within the 
offset distance.  This option applies to the PLANAR wall only.
*RIGIDWALL 
Tail of normal vector is the origin and
corner point if extent of stonewall is finite.
Figure 35-2.  Vector 𝐧 is normal to the rigidwall.  An optional vector 𝐥 can be
defined such that 𝐦 = 𝐧 × 𝐥.  The extent of the rigidwall is limited by defining
L  (LENL)  and  M  (LENM).    A  zero  value  for  either  of  these  lengths  indicates
that the rigidwall is infinite in that direction. 
  VARIABLE   
DESCRIPTION
BIRTH 
DEATH 
RWKSF 
Birth  time of  rigid  wall.    The  time  values  of the  load  curves  that
control the motion of the wall are offset by the birth time. 
Death time of rigid wall.  At this time the wall is deleted from the 
calculation.  If dynamic relaxation is active at the beginning of the
calculation  and  if  BIRTH = 0.0,  the  death  time  is  ignored  during 
the dynamic relaxation. 
Stiffness  scaling  factor.    If  RWKSF  is  also  specified  in  *CON-
TROL_CONTACT,  the  stiffness  is  scaled  by  the  product  of  the
two values. 
  Card 3 
Variable 
1 
XT 
Type 
F 
Default 
0. 
2 
YT 
F 
0. 
3 
ZT 
F 
0. 
4 
XH 
F 
0. 
5 
YH 
F 
0. 
6 
ZH 
F 
0. 
7 
8 
FRIC 
WVEL 
F 
0. 
F 
0.
VARIABLE   
DESCRIPTION
XT 
YT 
ZT 
XH 
YH 
ZH 
𝑥-coordinate  of  tail  of  any  outward  drawn  normal  vector,  𝐧, 
originating  on  wall  (tail)  and  terminating  in  space  (head),  see
Figure 35-2. 
𝑦-coordinate of tail of normal vector 𝐧 
𝑧-coordinate of tail of normal vector 𝐧 
𝑥-coordinate of head of normal vector 𝐧 
𝑦-coordinate of head of normal vector 𝐧 
𝑧-coordinate of head of normal vector 𝐧 
FRIC 
Coulomb friction coefficient except as noted below. 
EQ.0.0: frictionless sliding after contact, 
EQ.1.0: no sliding after contact, 
EQ.2.0: node  is  welded  after  contact  with  frictionless  sliding.
Welding  occurs  if  and  only  if  the  normal  value  of  the
impact  velocity  exceeds  the  critical  value  specified  by 
WVEL. 
EQ.3.0: node is welded after contact with no sliding.  Welding
occurs if and only if the normal value of the impact ve-
locity exceeds the critical value specified by WVEL. 
In  summary,  FRIC  could  be  any  positive  value.    Three  special 
values of FRIC trigger special treatments as follows: 
FRIC 
1.0 
2.0 
3.0 
Bouncing back from wall 
allowed 
not allowed 
not allowed 
Sliding on wall 
not allowed 
allowed 
not allowed 
WVEL 
Critical normal velocity at which nodes weld to wall (FRIC = 2 or 
3).
input
Node 2
points from
node 1 to 2
Node 1
defintion by nodes
b = n × d
a = b × n
definition by
vector components
Figure  35-3.    Definition  of  orthotropic  friction  vectors.    The  two  methods  of
defining the vector, 𝐝, are shown.  If vector 𝐝 is defined by nodes 1 and 2, the
local  coordinate  system  may  rotate  with  the  body  which  contains  the  nodes;
otherwise,  𝐝  is  fixed  in  space,  thus  on  the  rigid  wall,  and  the  local  system  is
stationary. 
Orthotropic Friction Card 1.  Additional card for ORTHO keyword option.  See Figure 
35-3 for the definition of orthotropic friction.  
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SFRICA 
SFRICB 
DFRICA 
DFRICB 
DECAYA  DECAYB 
Type 
F 
Default 
0. 
F 
0. 
F 
0 
F 
0 
F 
0. 
F 
0. 
Orthotropic Friction Card 2.  Additional card for ORTHO keyword option.  See Figure 
35-3 for the definition of orthotropic friction. 
  Card 5 
1 
2 
Variable 
NODE1 
NODE2 
Type 
I 
Default 
0. 
I 
0. 
3 
D1 
F 
0 
4 
D2 
F 
0 
5 
D3 
F 
0. 
6 
7 
8 
  VARIABLE   
DESCRIPTION
SFRICA 
SFRICB 
LS-DYNA R10.0 
Static friction coefficient in local a-direction, 𝜇𝑠𝑎, see Figure 35-3
VARIABLE   
DESCRIPTION
DFRICA 
Dynamic friction coefficient in local 𝑎-direction, 𝜇𝑘𝑎 
DFRICB 
Dynamic friction coefficient in local 𝑏-direction, 𝜇𝑘𝑏 
DECAYA 
Decay constant in local 𝑎-direction, 𝑑𝑦𝑎 
DECAYB 
Decay constant in local 𝑏-direction, 𝑑𝑦𝑏 
NODE1 
Node 1, alternative to definition with vector 𝐝 below.  See Figure 
35-3.  With the node definition the direction changes if the nodal
pair rotates. 
NODE2 
Node 2 
𝑑1,  𝑥-component  of  vector,  alternative  to  definition  with  nodes
above.  See Figure 35-3.  This vector is fixed as a function of time. 
𝑑2, 𝑦-component of vector 
𝑑3, 𝑧-component of vector 
D1 
D2 
D3 
Remarks: 
1.  The coefficients of friction are defined in terms of the static, dynamic and decay 
coefficients and the relative velocities in the local a and b directions as 
𝜇𝑎 = 𝜇𝑘𝑎 + (𝜇𝑠𝑎𝜇𝑘𝑎)𝑒𝑑𝑣𝑎𝑉relative,𝑎 
𝜇𝑏 = 𝜇𝑘𝑏 + (𝜇𝑠𝑏𝜇𝑘𝑏)𝑒𝑑𝑣𝑏𝑉relative,𝑏 
2.  Orthotropic  rigid  walls  can  be  used  to  model  rolling  objects  on  rigid  walls 
where  the  frictional  forces  are  substantially  higher  in  a  direction  transverse  to 
the rolling direction.  To use this option define a vector 𝒅 to determine the local 
frictional directions via: 
𝐛 = 𝐧 × 𝐝,
𝐚 = 𝐛 × 𝐧 
where 𝐧 is the normal vector to the rigid wall.  If 𝐝 is in the plane of the rigid 
wall, then 𝐚 is identical to 𝐝.
Finite  Wall  Size  Card.    Additional  card  for  FINITE  keyword  option.    See  Figure  35-3
for the definition of orthotropic friction.  See Figure 35-2.  The 𝒎 vector is computed as 
the vector cross product 𝒎 = 𝒏 × 𝒍.  The origin, the tail of the normal vector, is taken as 
the corner point of the finite size plane.  
  Card 6 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
XHEV 
YHEV 
ZHEV 
LENL 
LENM 
Type 
F 
Default 
0. 
F 
0. 
F 
F 
F 
0. 
infinity 
infinity 
  VARIABLE   
DESCRIPTION
XHEV 
YHEV 
ZHEV 
LENL 
x-coordinate of head of edge vector 𝒍, see Figure 35-2. 
y-coordinate of head of edge vector 𝒍 
z-coordinate of head of edge vector 𝒍 
Length of 𝒍 edge 
LENM 
Length of 𝒎 edge 
Moving  Wall  Card.    Additional  card  for  MOVING  keyword  option.    Note:  The 
MOVING option is not compatible with the ORTHO option. 
3 
4 
5 
6 
7 
8 
  Card 7 
1 
Variable 
MASS 
Type 
F 
2 
V0 
F 
Default 
none 
0. 
  VARIABLE   
DESCRIPTION
MASS 
Total mass of rigidwall 
V0 
Initial velocity of rigidwall in direction of defining vector, n
Forces  Card.    Additional  card  for  FORCES  keyword  option.    This  option  allows  the 
force  distribution  to  be  monitored  on  the  plane.    Also  four  points  can  be  defined  for 
visualization  of  the  rigid  wall.    A  shell  or  membrane  element  must  be  defined  with 
these four points as the connectivity for viewing in LS-PREPOST.  
7 
8 
  Card 7 
1 
2 
Variable 
SOFT 
SSID 
Type 
Default 
I 
0 
Remarks 
I 
0 
1 
3 
N1 
I 
0 
2 
4 
N2 
I 
0 
5 
N3 
I 
0 
6 
N4 
I 
0 
  VARIABLE   
DESCRIPTION
SOFT 
SSID 
Number of cycles to zero relative velocity to reduce force spike 
Segment  set  identification  number  for  defining  areas  for  force
output, see *SET_SEGMENT and remark 1 below. 
N1-N4 
Optional node for visualization 
Remarks: 
1.  The segment set defines areas for computing resultant forces.  These segments 
translate  with  the  moving  rigidwall  and  allow  the  forced  distribution  to  be 
determined.  The resultant forces are written in file “RWFORC.” 
2.  These four nodes are for visualizing the movement of the wall, i.e., they move 
with the wall.  To view the wall in LS-PREPOST it is necessary to define a single 
shell element with these four nodes as its connectivity.  The single element must 
be  deformable  (non  rigid)  or  else  the  segment  will  be  treated  as  a  rigid  body 
and the nodes will have their motion modified independently of the rigidwall.
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *RIGIDWALL_PLANAR_MOVING_FORCES 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Define a moving planar rigid wall: 
$     - that is parallel to the y-z plane starting at x = 250 mm 
$     - with an initial velocity of 8.94 mm/ms in the negative z-direction 
$     - that has a mass of 800 kg 
$     - which prevents all nodes in the model from penetrating the wall 
$     - with a friction coefficient for nodes sliding along the wall of 0.1 
$     - track the motion of the wall by creating a node (numbered 99999) 
$         at the tail of the wall and assigning the node to move with the wall 
$ 
*RIGIDWALL_PLANAR_MOVING_FORCES 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$     nsid    nsidex     boxid 
         0         0         0 
$ 
$       xt        yt        zt        xh        yh        zh      fric 
     250.0       0.0       0.0       0.0       0.0       0.0       0.1 
$ 
$  SW mass    SW vel 
    800.00      8.94 
$ 
$     soft      ssid     node1     node2     node3     node4 
         0         0     99999 
$ 
$ 
*NODE 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$    nid               x               y               z      tc      rc 
   99999           250.0             0.0             0.0       0       0 
$ 
$ 
*DATABASE_HISTORY_NODE 
$   Define nodes that output into nodout  
$      id1       id2       id3 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
     99999 
$       
*DATABASE_NODOUT 
$       dt 
       0.1 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
In  this  section,  the  element  formulation,  integration  rule,  nodal  thicknesses,  and  cross 
sectional properties are defined.  All section identifiers (SECID’s) defined in this section 
must  be  unique,  i.e.,  if  a  number  is  used  as  a  section  ID  for  a  beam  element  then  this 
number cannot be used again as a section ID for a solid element.  The keyword cards in 
this section are defined in alphabetical order: 
*SECTION_ALE1D 
*SECTION_ALE2D 
*SECTION_BEAM_{OPTION} 
*SECTION_BEAM_AISC 
*SECTION_DISCRETE 
*SECTION_POINT_SOURCE 
*SECTION_POINT_SOURCE_MIXTURE 
*SECTION_SEATBELT 
*SECTION_SHELL_{OPTION} 
*SECTION_SOLID_{OPTION} 
*SECTION_SPH_{OPTION} 
*SECTION_TSHELL 
The location and order of these cards in the input file are arbitrary. 
An additional option TITLE may be appended to all the *SECTION keywords.  If this 
option is used then an addition line is read for each section in 80a format which can be 
used to describe the section.  At present LS-DYNA does make use of the title.  Inclusion 
of titles gives greater clarity to input decks.
*SECTION_ALE1D 
Purpose:  Define section properties for 1D ALE elements 
Card Sets.  For each ALE1D section add one pair of cards 1 and 2.  This input ends at 
the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SECID 
ALEFORM 
AET 
ELFORM 
I 
none 
4 
5 
6 
7 
8 
I 
0 
3 
Type 
I/A 
I 
Default 
none 
none 
  Card 2 
1 
2 
Variable 
THICK 
THICK 
Type 
F 
F 
Default 
none 
none 
  VARIABLE   
SECID 
DESCRIPTION
Section  ID.    SECID  is  referenced  on  the  *PART  card.    A  unique 
number or label must be specified. 
ALEFORM 
ALE formulation: 
EQ.11:  Multi-Material ALE formulation.   
AET 
Ambient Element Type 
EQ.4: Pressure inflow 
ELFORM 
Element formulation: 
EQ.7:  Plane strain 
EQ.8:  Axisymmetric (per radian) 
EQ.-8:  spherical (per unit of solid angle)
VARIABLE   
DESCRIPTION
THICK 
Nodal thickness.  See Remark 1 
Remarks: 
1. 
*SECTION_ALE1D  is  using  the  common  *SECTION_BEAM  reader  which 
expects two thickness values.  However, the ALE 1D will simply take the aver-
age of these two values as the beam thickness.  
The thickness is not used for ELFORM = -8 but the reader routine expects val-
ues on the 2nd line.
*SECTION_ALE2D 
Purpose:  Define section properties for 2D ALE elements.  This supersedes the old way 
of defining section properties for 2D ALE elements via *SECTION_SHELL. 
For  coupling  between  2D  Lagrangian  elements  and  2D  ALE  elements,  use  *CON-
STRAINED_LAGRANGE_IN_SOLID rather than *CONTACT_2D_AUTOMATIC_SUR-
FACE_IN_CONTINUUM.   
In the case of an axisymmetric analysis, ELFORM for *SECTION_ALE2D can only be set 
to 14 (area-weighted).  In the same analysis, axisymmetric Lagrangian elements are not 
restricted to an area-weighted formulation.  In other words, shell formulation 14 or 15 
are permitted for Lagrangian shells and beam formulation 8 is permitted for Lagrangian 
beams.    Coupling  forces  between  the  axisymmetric  ALE  elements  and  axisymmetric 
Lagrangian elements are automatically adjusted as needed. 
Section Cards.  For each ALE2D section include a card.   This input terminates at the 
next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SECID 
ALEFORM 
AET 
ELFORM 
Type 
I/A 
I 
Default 
none 
none 
I 
0 
I 
none 
  VARIABLE   
SECID 
DESCRIPTION
Section  ID.    SECID  is  referenced  on  the  *PART  card.    A  unique
number or label must be specified. 
ALEFORM 
ALE formulation: 
EQ.11:  Multi-Material ALE formulation.
VARIABLE   
DESCRIPTION
AET 
Part type flag 
EQ.0:  This is a regular or non-ambient part (default) 
EQ.4:  Reservoir or ambient type part 
EQ.5:  Reservoir  or  ambient  type  part,  but  only  used  together
with *LOAD_BLAST_ENHANCED (LBE).  It defines this 
part as an “ambient receptor part” for the transient blast
load  supplied  by  a  corresponding  LBE  KW  . 
ELFORM 
Element formulation: 
EQ.13:  Plane strain (x-y plane) 
EQ.14:  Axisymmetric  solid  (x-y  plane,  y-axis  of  symmetry)  –
area weighted
*SECTION_BEAM_{OPTION} 
Available options include: 
<BLANK> 
AISC 
such that the keyword cards appear: 
*SECTION_BEAM 
*SECTION_BEAM_AISC 
Purpose:    Define  cross  sectional  properties  for  beam,  truss,  discrete  beam,  and  cable 
elements. 
The  AISC  option  may  be  used  to  specify  standard  steel  sections  as  specified  by  the 
American Institute of Steel Construction, and is described separately after *SECTION_-
BEAM 
Card Sets.  For each BEAM section in the model add one set of the following 2 (maybe 
3 for ELFORM = 12) cards.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SECID 
ELFORM 
SHRF 
QR/IRID 
CST 
SCOOR 
NSM 
Type 
I/A 
Default 
none 
I 
1 
F 
F 
F 
F 
F 
1.0 
2.0 
0.0 
0.0 
0.0 
Integrated Beam Card (types 1 and 11).  Card 2 for ELFORM set to either type 1 or 
11. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TS1 
TS2 
TT1 
TT2 
NSLOC 
NTLOC 
Type 
F 
F 
F 
F 
F
Resultant Beam With Shape Card (types 2, 3, and 12).  Card 2 for ELFORM equal to 
2, 3, or 12 and when first 7 characters of the card spell out “SECTION”. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  STYPE 
D1 
D2 
D3 
D4 
D5 
D6 
Type 
A10 
F 
F 
F 
F 
F 
Resultant Beam Card 1 (types 2, 12, and 13).  Card 2 for ELFORM equal to 2, 12, or 
13 and when first 7 characters of card do not spell “SECTION”. 
  Card 2 
Variable 
Type 
1 
A 
F 
2 
3 
ISS 
ITT 
F 
F 
4 
J 
F 
5 
6 
7 
8 
SA 
IST 
F 
F 
Resultant Beam Card 2 (type 12 only).  Card 3 for ELFORM equal to 12 and when first 
7 characters of card 2 do not spell “SECTION”. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
YS 
ZS 
IYR 
IZR 
IRR 
IW 
IWR 
Type 
F 
F 
F 
F 
F 
F 
F 
Resultant Beam Card (type 3).  Card 2 for ELFORM equal to 3. 
  Card 2 
Variable 
Type 
1 
A 
F 
2 
3 
4 
5 
6 
7 
8 
RAMPT  STRESS
F
Integrated Beam Card (types 4 and 5).  Card 2 for ELFORM equal to 4 or 5. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TS1 
TS2 
TT1 
TT2 
Type 
F 
F 
F 
F 
Discrete  Beam  Card  (type  6).    Card  2  for  ELFORM  equal  to  6  for  any  material other
than material type 146. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VOL 
INER 
CID 
CA  OFFSET RRCON  SRCON  TRCON
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Discrete  Beam Card  (type 6, mat 146).  Card  2  for  ELFORM  equal  to  6  for  material 
type 146. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VOL 
INER 
CID 
DOFN1 DOFN2
Type 
F 
F 
F 
F 
F 
2D Shell Card (types 7 and 8).  Card 2 for ELFORM equal to 7 or 8. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TS1 
TS2 
TT1 
TT2 
Type 
F 
F 
F
Spot Weld Card (type 9).  Card 2 for ELFORM equal to 9. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TS1 
TS2 
TT1 
TT2 
PRINT 
Type 
F 
F 
F 
F 
F 
Integrated Beam Card (types 14).  Card 2 for ELFORM equal to 14. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PR 
IOVPR 
IPRSTR
Type 
F 
F 
F 
F 
  VARIABLE   
SECID 
DESCRIPTION
Section  ID.    SECID  is  referenced  on  the  *PART  card.    A  unique
number or label must be specified. 
ELFORM 
Element formulation options: 
EQ.1:  Hughes-Liu with cross section integration (default), 
EQ.2:  Belytschko-Schwer resultant beam (resultant), 
EQ.3: 
truss (resultant).  See Remark 2. 
EQ.4:  Belytschko-Schwer full cross-section integration, 
EQ.5:  Belytschko-Schwer  tubular  beam  with  cross-section 
integration, 
EQ.6:  discrete beam/cable, 
EQ.7:  2D plane strain shell element (𝑥𝑦 plane), 
EQ.8:  2D  axisymmetric  volume  weighted  shell  element  (𝑥𝑦
plane, 𝑦-axis of symmetry), 
EQ.9:  spotweld beam, see *MAT_SPOTWELD. 
EQ.11:  integrated warped beam.  See Remark 4) 
EQ.12:  resultant warped beam 
EQ.13:  small displacement, linear Timoshenko beam with exact
stiffness.  See Remark 6 
EQ.14:  Elbow  integrated  tubular  beam  element.    An  user
VARIABLE   
DESCRIPTION
SHRF 
QR/IRID 
defined  integration  rule  with  tubular  cross  section  (9) 
must be used. 
Note  that  the  2D  and  3D  element  types  must  not  be  mixed,  and
different  types  of  2D  elements  must  not  be  used  together.    For
example, the plane strain element type must not be used with the
axisymmetric  element  type.    In  3D  the  different  beam  elements
types, i.e., 1-6 and 9 can be freely mixed together. 
Shear  factor.    This  factor  is  not  needed  for  truss,  resultant  beam,
discrete  beam,  and  cable  elements.    The  recommended  value  for
rectangular sections is 5/6, the default is 1.0. 
Quadrature  rule  or  rule  number  for  user  defined  rule  for
integrated beams.  See Remark 10 regarding beam formulations 7 
and 8. 
EQ.1.0: one integration point, 
EQ.2.0: 2 × 2 Gauss quadrature (default beam), 
EQ.3.0: 3 × 3 Gauss quadrature, 
EQ.4.0: 3 × 3 Lobatto quadrature, 
EQ.5.0: 4 × 4 Gauss quadrature 
EQ.-n:  where  |n|  is  the  number  of  the  user  defined  rule.
IRID  integration  rule  n  is  defined  using  *INTEGRA-
TION_BEAM card. 
CST 
Cross section type, not needed for truss, resultant beam, discrete
beam, and cable elements: 
EQ.0.0: rectangular, 
EQ.1.0: tubular (circular only), 
EQ.2.0: arbitrary (user defined integration rule). 
SCOOR 
Affects the discrete beam formulation  and also the 
update  of  the  local  coordinate  system  of  the  discrete  beam
element.    This  parameter  does  not  apply  to  cable  elements.    The
force  and  moment  resultants  in  the  output  databases  are  output
in  the  local  coordinate  system.    See  Remark  9  for  more  on  the 
local coordinate system update.   
EQ.-13.0:  Like -3.0, but with correction for beam rotation
VARIABLE   
DESCRIPTION
EQ.-12.0:  Like -2.0, but with correction for beam rotation
EQ.-3.0:  beam  node  1,  the  angular  velocity of  node 1  rotates
triad, 
EQ.-2.0:  beam  node  1,  the  angular  velocity of  node 1  rotates
triad  but  the  r-axis  is  adjusted  to  lie  along  the  line 
between the two beam nodal points.   This  option is
not recommended for zero length discrete beams., 
EQ.-1.0:  beam  node  1,  the  angular  velocity of  node 1  rotates
triad, 
EQ.0.0: 
centered  between  beam  nodes  1  and  2,  the  average 
angular  velocity  of  nodes  1  and  2  is  used  to  rotate
the triad, 
EQ.+1.0:  beam  node  2,  the  angular  velocity of  node 2  rotates
triad. 
EQ.+2.0:  beam  node  2,  the  angular  velocity of  node 2  rotates
triad.  but the r-axis is adjusted to lie along the line 
between the two beam nodal points.   This  option is
not recommended for zero length discrete beams. 
EQ.+3.0:  beam  node  2,  the  angular  velocity of  node 2  rotates
triad. 
EQ.+12.0:  Like +2.0, but with correction for beam rotation 
EQ.+13.0:  Like +3.0, but with correction for beam rotation 
Nonstructural mass per unit length.  This option applies to beam
types 1-5 and does not apply to discrete, 2D, and spotweld beams,
respectively. 
Beam thickness (CST = 0.0, 2.0) or outer diameter (CST = 1.0) in s 
direction at node 𝑛!.  Note that the thickness defined on the *ELE-
MENT_BEAM_THICKNESS  card  overrides  the  definition  give 
here.  Thickness at node 𝑛1  for beam formulations 7 and 8. 
Beam thickness (CST = 0.0, 2.0) or outer diameter (CST = 1.0) in s 
direction  at  node  𝑛2.    For  truss  elements  only,  it  is  the  ramp  up 
time for the stress initialization by dynamic relaxation.  Thickness
at node 𝑛2  for beam formulations 7 and 8. 
NSM 
TS1 
TS2
VARIABLE   
DESCRIPTION
TT1 
TT2 
Beam thickness (CST = 0.0, 2.0) or inner diameter (CST = 1.0) in t 
direction  at  node  𝑛1.    For  truss  elements  only,  it  is  the  stress  for 
the initialization of the stress by dynamic relaxation.  Not used by
beam formulations 7 and 8. 
Beam thickness (CST = 0.0, 2.0) or inner diameter (CST = 1.0) in t 
direction at node 𝑛2.  Not used by beam formulations 7 and 8. 
NSLOC 
Location  of  reference  surface  normal  to  𝑠  axis  for  Hughes-Liu 
beam elements only.  See Remark 5. 
EQ.1.0:  side at 𝑠 = 1.0, 
EQ.0.0:  center, 
EQ.-1.0:  side at 𝑠 = −1.0. 
NTLOC 
Location  of  reference  surface  normal  to  𝑡  axis  for  Hughes-Liu 
beam elements only.  See Remark 5. 
EQ.1.0:  side at 𝑡 = 1.0, 
EQ.0.0:  center, 
EQ.-1.0:  side at 𝑡 = −1.0. 
A 
ISS 
ITT 
J 
SA 
Cross-sectional  area.    The  definition  on  *ELEMENT_BEAM_-
THICKNESS overrides the value defined here.  
𝐼𝑠𝑠,  area  moment  of  inertia  about  local  𝑠-axis.    The  definition  on 
*ELEMENT_BEAM_THICKNESS  overrides  the  value  defined 
here. 
𝐼𝑡𝑡,  area  moment  of  inertia  about  local  𝑡-axis.    The  definition  on 
*ELEMENT_BEAM_THICKNESS  overrides  the  value  defined 
here. 
𝐽,  torsional  constant.    The  definition  on  *ELEMENT_BEAM_
THICKNESS overrides the value defined here  If J is zero, then J is
reset  to  the  sum  of  ISS +  ITT  as  an  approximation  for  warped 
beam. 
Shear  area.    The  definition  on  *ELEMENT_BEAM_THICKNESS 
overrides the value defined here.
VARIABLE   
DESCRIPTION
IST 
YS 
ZS 
IYR 
IZR 
IRR 
IW 
IWR 
PR 
𝐼𝑠𝑡, product area moment of inertia w.r.t.  local 𝑠- and 𝑡-axis.  This 
is  only  non-zero  for  asymmetric  cross  sections  and  it  can  take 
positive and negative values, e.g.  it is negative for SECTION_03. 
𝑠  coordinate  of  shear  center  of  cross-section.    (The  coordinate 
system is located at the centroid.) 
𝑡  coordinate  of  shear  center  of  cross-section.    (The  coordinate 
system is located at the centroid.) 
∫ 𝑠𝑟2𝑑𝐴
, where 𝑟2 = 𝑠2 + 𝑡2 
∫ 𝑡𝑟2𝑑𝐴
, where 𝑟2 = 𝑠2 + 𝑡2 
∫ 𝑟4𝑑𝐴
, where 𝑟2 = 𝑠2 + 𝑡2 
Warping constant. ∫ 𝜔2𝑑𝐴
, where 𝜔 is the sectorial area. 
∫ 𝜔𝑟2𝑑𝐴
Pressure inside ELBOW elements that belong to the section.  The
pressure acts as a stiffener and will reduce the ovalization of the
pipe.  Pressure acting on the inside wall is taken as positive. 
IOVPR 
Print flag for the ELBOW ovalization degrees of freedom. 
EQ.1.0: an ascii file named elbwov is created and filled with the 
ovalization.  Default no file is created. 
IPRSTR 
Flag  for  adding  stress  due  to  pressure  PR  into  the  material
routine. 
EQ.0: No  stress  is  added  to  the  material.    In  this  case  the
pressure only acts as a stiffener for the tube. 
EQ.1: The pressure PR is used to calculate additional axial and
circumferential  stresses  due  to  the  applied  pressure  PR.
The stress added is given by: 
𝜎axial = PR ×
4𝑇
,
𝜎circ = pr ×
2𝑇
for a straight pipe, and 
𝜎axial = PR ×
4𝑇
,
𝜎circ = PR ×
4𝑇
[2𝑅 + 𝑟 cos(𝜃)]
[𝑅 + 𝑟 cos(𝜃)]
for a curved pipe.  D is the pipe diameter, T is the thickness, R is
VARIABLE   
DESCRIPTION
RAMPT 
STRESS 
the curvature of the bend, r is the pipe radius (mean) and θ is an 
angle  pointing  out  a  point  on  the  pipe.    EQ.1  also  includes  the
stiffening effect.  
Optional ramp-up time for dynamic relaxation.  At the end of the
ramp-up time, a uniform stress, STRESS, will exist in the truss in
the  truss  element.    This  option  will  not  work  for  hyperelastic
materials. 
Optional  initial  stress  for  dynamic  relaxation.    At  the  end  of 
dynamic  relaxation  a  uniform  stress  equal  to  this  value  should
exist in the truss element. 
STYPE 
Section type (A format) of resultant beam, see Figure 36-1: 
EQ.SECTION_01: I-Shape 
EQ.SECTION_02: Channel 
EQ.SECTION_03: L-shape 
EQ.SECTION_04: T-shape 
EQ.SECTION_05: Tubular box 
EQ.SECTION_06: Z-Shape 
EQ.SECTION_07: Trapezoidal 
EQ.SECTION_08: Circular 
EQ.SECTION_09: Tubular 
EQ.SECTION_10: I-Shape 2 
EQ.SECTION_11: Solid Box 
EQ.SECTION_12:  Cross 
EQ.SECTION_13:  H-Shape 
EQ.SECTION_14:  T-Shape 2 
EQ.SECTION_15:  I-Shape 3 
EQ.SECTION_16:  Channel 2 
EQ.SECTION_17:  Channel 3 
EQ.SECTION_18:  T-Shape 3 
EQ.SECTION_19:  Box-Shape 2
EQ.SECTION_20:  Hexagon 
EQ.SECTION_21:  Hat-Shape 
EQ.SECTION_22:  Hat-Shape 2 
D1-D6 
Input parameters for section option using STYPE above. 
VOL 
Volume  of  discrete  beam  and  scalar  (MAT_146)  beam.    Used  in 
calculating  mass.    If  VOL = 0  for  cable  elements,  volume  is 
calculated  as  the  product  of  cable  length  and  cable  area.    If  the
mass density of the material model for the discrete beam is set to
unity,  the  magnitude  of  the  lumped  mass  can  be  defined  here 
instead.  This lumped mass is partitioned to the two nodes of the
beam  element.    The  translational  time  step  size  for  the  type  6
beam  is  dependent  on  the  volume,  mass  density,  and  the
translational  stiffness  values,  so  it  is  important  to  define  this 
parameter.  Defining the volume is also essential for mass scaling
if the type 6 beam controls the time step size.
INER 
CID 
CA 
OFFSET 
*SECTION 
DESCRIPTION
Mass  moment  of  inertia  for  the  six  degree  of  freedom  discrete
beam  and  scalar  (MAT_146)  beam.    This  parameter  does  not 
apply to cable elements.  This lumped inertia is partitioned to the
two nodes of the beam element.  The rotational time step size for
the  type  6  beam  is  dependent  on  the  lumped  inertia  and  the
rotational  stiffness  values,  so  it  is  important  to  define  this
parameter  if  the  rotational  springs  are  active.    Defining  the
rotational  inertia  is  also  essential  for  mass  scaling  if  the  type  6
beam  rotational  stiffness  controls  the  time  step  size.    It  is
recommended  to  always  set  this  parameter  to  a  reasonable
nonzero  value  to  avoid  instabilities  and/or  having  model
dependent rotational inertia properties, if the value set is smaller
than  that  of  an  equivalent  solid  sphere  LS-DYNA  will  issue  a 
warning. 
Coordinate system ID for orientation (material types 66-69, 93, 95, 
97),  see  *DEFINE_COORDINATE_option.    If  CID = 0,  a  default 
coordinate system is defined in the global system or on the third
node  of  the  beam,  which  is  used  for  orientation.    This  option  is
not defined for material types than act between two nodal points, 
such  as  cable  elements.    The  coordinate  system  rotates  with  the
discrete beam, see SCOOR above. 
Cable  area.    See  material  type  71,  *MAT_CABLE_DISCRETE_-
BEAM. 
Optional  offset  for  cable.    See  material  type  71,  *MAT_CABLE_-
DISCRETE_BEAM. 
RRCON 
𝑟-rotational constraint for local coordinate system 
EQ.0.0: Coordinate ID rotates about 𝑟 axis with nodes. 
EQ.1.0: Rotation is constrained about the 𝑟-axis 
SRCON 
𝑠-rotational constraint for local coordinate system 
EQ.0.0: Coordinate ID rotates about 𝑠 axis with nodes. 
EQ.1.0: Rotation is constrained about the 𝑠-axis 
TRCON 
𝑡-rotational constraint for local coordinate system  
EQ.0.0: Coordinate ID rotates about 𝑡 axis with nodes. 
EQ.1.0: Rotation is constrained about the 𝑡-axis
CID 
*SECTION_BEAM 
DESCRIPTION
Coordinate system ID for orientation, material type 146, see *DE-
FINE_COORDINATE_SYSTEM.    If  CID = 0,  a  default  coordinate 
system is defined in the global system. 
DOFN1 
Active  degree-of-freedom  at  node  1,  a  number  between  1  and  6
where 1 in 𝑥-translation and 4 is 𝑥-rotation. 
DOFN2 
Active degree-of-freedom at node 2, a number between 1 and 6. 
PRINT 
Output spot force resultant from spotwelds. 
EQ.0.0: Data is output to swforc file. 
EQ.1.0: Output is suppressed. 
Remarks: 
1. 
Implicit  Time  Integrator.    For  implicit  calculations  all  of  the  beam  element 
choices are implemented: 
2.  Truss Elements.  For the truss element, define the cross-sectional area, 𝐴, only. 
3.  Local  Coordinate  System  Rotation.    The  local  coordinate  system  rotates  as 
the  nodal  points  that  define  the  beam  rotate.    In  some  cases  this  may  lead  to 
unexpected  results  if  the  nodes  undergo  significant  rotational  motions.    In  the 
definition  of  the  local  coordinate  system  using  *DEFINE_COORDINATE_-
NODES, if the option to update the system each cycle is active then this updat-
ed  system  is  used.    This  latter  technique  seems  to  be  more  stable  in  some 
applications. 
4. 
Integrated Warped Beam.  The integrated warped beam (type 11) is a 7 degree 
of freedom beam that must be used with an integration rule of the open stand-
ard cross sections, see *INTEGRATION_BEAM.  To incorporate the additional 
degrees  of  freedom  corresponding  to  the  twist  rates,  the  user  should  declare 
one scalar node (*NODE_SCALAR) for each node attached to a warped beam.  
This  degree  of  freedom  is  associated  to  the  beam  element  using  the  warpage 
option on the *ELEMENT_BEAM card. 
5.  Beam  Offsets.    Beam  offsets  are  sometimes  necessary  for  correctly  modeling 
beams that act compositely with other elements such as shells or other beams.  
A beam offset extends from the beam’s 𝑛1-to-𝑛2 axis to the reference axis of the 
beam.  The beam reference axis lies at the origin of the local 𝑠 and 𝑡 axes.  This 
origin  is  located  at  the  center  of  the  cross-section  footprint  for  beam  formula-
tions  1  and  11  but  it  is  located  at  the  cross-section  centroid  for  beam  formula-
tion  2.    Note  that  for  cross-sections  that  are  not  doubly  symmetric,  e.g,  a  T-
section,  the  center  of  the  cross-section  footprint  and  the  centroid  of  the  cross-
section do not coincide.  The offset in the positive 𝑠-direction is 
s-offset  =   −0.5 ×  NSLOC
× (beam cross-section dimension in 𝑠-direction). 
Similarly, the offset in the positive t-direction is 
t-offset  =   −0.5 ×  NTLOC
× (beam cross-section dimension in 𝑡-direction). 
If IRID is used to point to an integration rule with ICST > 0, then offsets must be 
defined using SREF and TREF on the *INTEGRATION_BEAM card as they will 
override  NSLOC  and  NTLOC  even  if  SREF = 0  or  TREF = 0.    See  also 
*ELEMENT_BEAM_OFFSET for an alternate approach to defining beam offsets. 
6.  3-D Timoshenko Beam.  Element type 13 is a 3-D Timoshenko resultant-based 
beam element with two nodes for small displacement, linear isotropic elasticity.  
The stiffness matrix is identical to the residual stiffness formulation used in the 
Belytschko-Schwer  element  (type  2).    This  element  only  works  with  *MAT_-
ELASTIC.  It uses the reference geometry to calculate the element stiffness and 
calculates  the  element  forces  by  multiplying  the  element  stiffness  by  the  dis-
placements.    Offsets  work  but  they  are fixed  for  all  time  like  the reference  ge-
ometry. 
7.  SCOOR.    If  the  magnitude  of  SCOOR  is  less  than  or  equal  to  unity  then  zero 
length  discrete  beams  are  assumed  with  infinitesimal  separation  between  the 
nodes in the deformed state.  For large separations or nonzero length beams set 
|SCOOR| to 2, 3, 12, or 13, in which case true beam-like behavior is invoked to 
provide equilibrating torques to offset any force couples that arise due to trans-
lational  stiffness  or  translational  damping.    Also,  rigid  body  rotation  is  meas-
ured  and  the  spring  strain  modified  so  that  rotation  does  not  create  strain.    A 
flaw in this strain modification was found in the implementation of |SCOOR| 
= 2 and 3 the improved formulation is activated by setting |SCOOR| = 12 and 
13.  The original options were left in place to allow legacy data to run without 
change. 
8.  Disabling  Nodal  Rotations.    RRCON,  SRCON,  and  TRCON  are optional  and 
apply  only  to  non-cable  discrete  beams.    If  set  to  1,  RRCON,  SRCON,  and 
TRCON  will  prevent  nodal  rotations  about  the  local  𝑟,  𝑠,  𝑡  axes,  respectively, 
from affecting the update of the local coordinate system.  These three parame-
ters have no influence on how nodal translations may affect the local coordinate 
system update.
9.  Note  about  Local  Coordinate  Updates  and  FLAG.    If  CID  is  nonzero  for  a 
discrete beam and the coordinate system identified by CID uses *DEFINE_CO-
ORDINATE_NODES with FLAG=1, the beam local system is updated based on 
the  current  orientation  of  the  three  nodes  identified  in  *DEFINE_COORDI-
NATE_NODES.  In this case, local coordinate system updates per SCOOR types 
0,  ±1,  ±3,  and  ±13  are  inactive  while  for  SCOOR  types  ±2  and  ±12,  a  final 
adjustment  is  made  to  the  local  coordinate  system  so  that  the  local  𝑟-axis  lies 
along  the  𝑛1-to-𝑛2  axis  of  the  beam.    An  optional  output  database  (*DATA-
BASE_DISBOUT) will report relative displacements, rotations, and force result-
ants of discrete beams, all in the local coordinate system. 
10.  Beams 7 and 8.  Beam formulations 7 and 8 are 2D shell elements.  For these 
two  formulations,  variable  QR/IRID  is  the  number  of  through  thickness  inte-
gration points for the shell.   Output for these integration points is controlled by 
the variable BEAMIP in *DATABASE_EXTENT_BINARY. 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *SECTION_BEAM 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Define a Belytschko-Schwer resultant beam (elform = 2) with the following 
$  properties.  This beam models the connection/stiffening beams of a medium 
$  size roadside sign. 
$ 
$    cross sectional area:                       a =     515.6 mm2 
$    2nd moment of area about s-axis:          iss =  99,660.0 mm4 
$    2nd moment of area about t-axis:          iss =  70,500.0 mm4 
$    2nd polar moment of area about beam axis:   j = 170,000.0 mm4 
$ 
*SECTION_BEAM 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      sid    elform      shrf   qr/irid       cst 
       111         2 
$ 
$        a       iss       itt         j        sa 
     515.6   99660.0   70500.0  170000.0 
$ 
*SECTION_BEAM_TITLE 
    Main beam member  
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      sid    elform      shrf   qr/irid       cst 
       111         2 
$ 
$        a       iss       itt         j        sa 
     515.6   99660.0   70500.0  170000.0 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
D3
D2
D4
D1
D4
D3
D1
D2
  Figure 36-1.  SECTION_01 ⇒ I-Shape 
  Figure 36-2.  SECTION_02 ⇒ Channel 
D4
D3
D1
D2
D3
D1
D2
D4
  Figure 36-3.  SECTION_03 ⇒ L-Shape 
  Figure 36-4.  SECTION_04 ⇒ T-Shape 
D3
D2
D1
D4
D1
D4
D3
D2
  Figure 36-5.  SECTION_05 ⇒ Box-Shape    Figure 36-6.  SECTION_06 ⇒ Z-Shape
D1
D3
D2
D1
Figure 36-7.  SECTION_07 ⇒ Trapezoidal-
  Figure 36-8.  SECTION_08 ⇒ Circular 
Shape 
D1
D2
D6
D5
D3
D2
D4
D1
  Figure 36-9.  SECTION_09 ⇒ Tubular 
  Figure 36-10.  SECTION_10 ⇒ I-Shape 2 
D2
D1
D4
D3
D1/2
D1/2
D2
Figure 36-11.  SECTION_11 ⇒ Solid Box    Figure 36-12.  SECTION_12 ⇒ Cross 
D2/2
D4
D2/2
D3
D4
D3
D1
D2
D1
  Figure 36-13.  SECTION_13 ⇒ H-Shape    Figure 36-14.  SECTION_14 ⇒ T-Shape 2
D1/2
D4
D2
D1/2
D3
D4
D1
D3
D2
  Figure 36-15.  SECTION_15 ⇒ I-Shape 3    Figure 36-16.  SECTION_16 ⇒ Channel 2
D1
D3
D1
D2
D4
D2
D4
D1
D3
Figure 36-17.  SECTION_17 ⇒ Channel 3   Figure 36-18.  SECTION_18 ⇒ T-Shape 3
D1
D2
D5
D3
D6
D2
D3
D4
D1
Figure  36-19.    SECTION_19  ⇒  Box-Shape 
  Figure 36-20.  SECTION_20 ⇒ Hexagon 
2 
D3
D1
D4
D2
D4
Figure 36-21.  SECTION_21 ⇒ Hat Shape
D2
D6
D4
D3
D1
D6
D5
Figure 36-22.  SECTION_22 ⇒ Hat Shape 2
*SECTION_BEAM_AISC 
Purpose:    Define  cross-sectional  properties  for  beams  and  trusses  using  section  labels 
from the AISC Steel Construction Manual, 2005, 13th Edition, as published in the AISC 
Shapes Database V13.1.1 
Card Sets.  For each BEAM_AISC section include one pair of cards 1 and 2.  This input 
ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SECID 
Type 
I 
LABEL 
A70 
Integrated Beam Card (types 1 and 11).  Card 2 for ELFORM equal to 1 or 11. 
  Card 2 
1 
2 
3 
4 
5 
6 
Variable 
ELFORM 
SHRF 
NSM 
LFAC 
NSLOC 
NTLOC 
Type 
I 
F 
F 
F 
F 
F 
8 
7 
K 
I 
Resultant Beam Card (types 2 and 12).  Card 2 for ELFORM equal to 2 or 12. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ELFORM 
SHRF 
NSM 
LFAC 
Type 
I 
F 
F 
F 
Truss Beam Card (type 3).  Card 2 for ELFORM equal to 3. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ELFORM 
LFAC 
RAMPT 
STRESS 
Type 
I 
F 
F
Integrated Beam Card (types 4 and 5).  Card 2 for ELFORM equal to 4 or 5. 
  Card 2 
1 
2 
3 
4 
Variable 
ELFORM 
SHRF 
NSM 
LFAC 
5 
K 
6 
7 
8 
Type 
I 
F 
F 
K 
  VARIABLE   
SECID 
DESCRIPTION
Section  ID.    SECID  is  referenced  on  the  *PART  card.    A  unique
number or label must be specified. 
LABEL 
AISC section label 
ELFORM 
Element  formulation  .    Only  types  1–
5,11,12 are allowed 
SHRF 
NSM 
LFAC 
Shear factor  
Non-structural mass per unit length 
GT.0.0:  Length  scale  factor  to  convert  dimensions  from  standard
units 
LT.0.0: Use predefined length factor for specific model units 
             EQ.-1.0: ft 
             EQ.-2.0: m 
             EQ.-3.0: in 
             EQ.-4.0: mm 
             EQ.-5.0: cm 
NSLOC 
Location of reference surface  
NTLOC 
Location of reference surface  
K 
Integration refinement parameter  
RAMPT 
Optional ramp-up time  
STRESS 
Optional initial stress
*SECTION_BEAM_AISC 
This keyword uses the dimensions of the standard AISC beams sections — as defined 
by the section label — to define *SECTION_BEAM and *INTEGRATION_BEAM cards 
with the appropriate parameters. 
The AISC section label may be specified either as the shape designation as seen in the 
AISC  Steel  Construction  Manual,  2005,  or  the  designation  according  to  the  AISC 
Naming Convention for Structural Steel Products for Use in Electronic Data Interchange 
(EDI), 2001.  As per the EDI convention, the section labels are to be case-sensitive and 
space  sensitive,  i.e.    “W36X150”  is  acceptable  but  “W36  x  150”  is  not.    Labels  can  be 
specified in terms of either the U.S.  Customary units (in) or metric units (mm), which 
will determine the length units for the section dimensions.  The parameter LFAC may 
be  used  as  a  multiplier  to  convert  the  dimensions  to  other  lengths  units.    For  user 
convenience,  predefined  conversion  factors  are  provided  for  specific  choices  of  the 
model length unit. 
AISC requires the following legal notice specifying that LS-DYNA users may not extract 
AISC shapes data in any manner from LS-DYNA to create commercial software.  Users 
are certainly allowed to create LS-DYNA input models for commercial purposes using 
this card. 
AISC FLOW-DOWN LICENSE TERMS (TERMS OF USE) 
This  application  contains  software  from  the  American  Institute  of  Steel  Construction, 
Inc.    of  Chicago,  Illinois  d/b/a  AISC  (“AISC”).    The  software  from  AISC  (the  “AISC 
Shapes  Database”)  enables  this  application  to  provide  dimensions  and  properties  of 
structural steel shapes and to perform other functions.  You may use AISC Data only by 
means of the intended End User functions of this application software.  You agree that 
you will use AISC Data for non-commercial use only, meaning that it will not be used to 
develop or create revenue-producing software.  You agree not to assign, copy, transfer 
or transmit the AISC Shapes Database or any AISC Data to any third party. 
YOU  AGREE  NOT  TO  USE  OR  EXPLOIT  AISC  DATA  OR  THE  AISC  SHAPES 
DATABASE EXCEPT AS EXPRESSLY PERMITTED HEREIN.
*SECTION 
Purpose:    Defined  spring  and  damper  elements  for  translation  and  rotation.    These 
definitions  must  correspond  with  the  material  type  selection  for  the  elements,  i.e., 
*MAT_SPRING_...  and *MAT_DAMPER_... 
Card Sets.  For each DISCRETE section include a pair of cards 1 and 2.  This input ends 
at the next keyword (“*”) card. 
3 
KD 
F 
3 
4 
V0 
F 
4 
5 
CL 
F 
5 
6 
FD 
F 
6 
7 
8 
7 
8 
  Card 1 
1 
2 
Variable 
SECID 
DRO 
Type 
I/A 
  Card 2 
1 
I 
2 
Variable 
CDL 
TDL 
Type 
F 
F 
  VARIABLE   
SECID 
DESCRIPTION
Section  ID.    SECID  is  referenced  on  the  *PART  card.    A  unique
number or label must be specified. 
DRO 
Displacement/Rotation Option: 
EQ.0: the material describes a translational spring/damper, 
EQ.1: the material describes a torsional spring/damper. 
Dynamic magnification factor.  See Remarks 1 and 2 below. 
Test velocity 
Clearance.  See Remark 3 below. 
Failure deflection (twist for DRO = 1).  Negative for compression, 
positive for tension. 
Deflection (twist for DRO = 1) limit in compression.  See Remark 
4 below. 
KD 
V0 
CL 
FD 
CDL
Deflection  (twist  for  DRO = 1)  limit  in  tension.    See  Remark  4 
below. 
*SECTION 
  VARIABLE   
TDL 
Remarks: 
1.  The constants from KD to TDL are optional and do not need to be defined. 
2. 
If kd is nonzero, the forces computed from the spring elements are assumed to 
be the static values and are scaled by an amplification factor to obtain the dy-
namic value: 
𝐹dynamic = (1. +𝑘𝑑
𝑉0
) 𝐹static 
where 
V  =  absolute value of the relative velocity between the nodes. 
V0  =  dynamic test velocity. 
For  example,  if  it  is  known  that  a  component  shows  a  dynamic  crush  force  at 
15m/s equal to 2.5 times the static crush force, use kd  = 1.5 and V0 = 15. 
3.  Here,  “clearance”  defines  a  compressive  displacement  which  the  spring 
sustains  before  beginning  the  force-displacement  relation  given  by  the  load 
curve  defined  in  the material  selection.   If a  non-zero  clearance  is  defined,  the 
spring is compressive only. 
4.  The deflection limit in compression and tension is restricted in its application to 
no more than one spring per node subject to this limit, and to deformable bod-
ies only.  For example in the former case, if three springs are in series, either the 
center spring or the two end springs may be subject to a limit, but not all three.  
When  the  limiting  deflection  is  reached,  momentum  conservation  calculations 
are  performed  and  a  common  acceleration  is  computed  in  the  appropriate  di-
rection.  An error termination will occur if a rigid body node is used in a spring 
definition where deflection is limited. 
Constrained boundary conditions on the *NODE cards and the BOUNDARY_-
SPC cards must not be used for nodes of springs with deflection limits. 
5.  Discrete elements can be included in implicit applications. 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *SECTION_DISCRETE 
$
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Note: These examples are in kg, mm, ms, kN units. 
$ 
$  A translational spring (dro = 0) is defined to have a failure deflection 
$  of 25.4 mm (fd = 25.4).  The spring has no dynamic effects or 
$  deflection limits, thus, those parameters are not set. 
$ 
*SECTION_DISCRETE 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      sid       dro        kd        v0        cl        fd 
       104         0                                    25.4 
$ 
$      cdl       tdl 
$ 
$ 
$  Define a translational spring that is known to have a dynamic crush force 
$  equal to 2.5 times the static force at a 15 mm/ms deflection rate. 
$  Additionally, the spring is known to be physically constrained to deflect 
$  a maximum of 12.5 mm in both tension and compression. 
$ 
*SECTION_DISCRETE 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      sid       dro        kd        v0        cl        fd 
       107         0       1.5      15.0 
$ 
$      cdl       tdl 
      12.5      12.5 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
*SECTION_POINT_SOURCE 
Purpose:    This  command  provides  the  inlet  boundary  condition  for  single  gas  in  flow 
(inflation  potential)  via  a  set  of  point  source(s).    It  also  provides  the  inflator  orifice 
geometry information.  It requires 3 curves defining the inlet condition for the inflator 
gas coming into the tank or an airbag as input (𝑇̅̅̅̅gas corrected(𝑡), 𝑣𝑟(𝑡), and vel(𝑡)).  Please 
see also the *ALE_TANK_TEST card for additional information. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SECID 
LCIDT 
LCIDVR 
LCIDVEL 
NIDLC1 
NIDLC2 
NIDLC3 
Type 
I/A 
Default 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
Source  Node  Cards.    Include  one  card  for  each  source  node.    This  input  ends  at  the 
next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NODEID 
VECID 
ORIFA 
Type 
Default 
I 
0 
I 
0 
F 
0.0 
  VARIABLE   
DESCRIPTION
SECID 
LCIDT 
Section ID.  A unique number or label must be specified. 
Temperature load curve ID 
LCIDVR 
Relative volume load curve ID 
LCIDVEL 
Inlet flow velocity load curve ID 
NIDLC1 
NIDLC2 
The 1st node ID defining a local coordinate . 
The 2nd node ID defining a local coordinate .
VARIABLE   
DESCRIPTION
NIDLC3 
The 3rd node ID defining a local coordinate . 
NODEID 
The node ID(s) defining the point source(s). 
VECID 
The vector ID defining the direction of flow at each point source. 
ORIFA 
The orifice area at each point source. 
Remarks: 
1. 
2. 
In  an  airbag  inflator  tank  test,  the  tank  pressure  data  is  measured.    This 
pressure is used to derive 𝑚̇ (𝑡) and the estimated 𝑇̅̅̅̅𝑔𝑎𝑠(𝑡), usually via a lumped-
parameter method, a system of conservation equations and EOS.  Subsequently 
𝑚̇ (𝑡)  and  𝑇̅̅̅̅𝑔𝑎𝑠(𝑡)    (stagnation  temperature)  are  used  as  input  to  obtain 
𝑇̅̅̅̅𝑔𝑎𝑠_ 𝑐𝑜𝑟𝑟𝑒𝑐𝑡𝑒𝑑(𝑡)  (static  temperature),  𝑣𝑟(𝑡),  and  𝑣𝑒𝑙(𝑡).    These  3  curves  are  then 
used  to  describe  inflator  gas  inlet  condition  . 
In a car crash model, the inflator housing may get displaced during the impact.  
The 3 node IDs defines the local reference coordinate system to which the point 
sources are attached.  These 3 reference nodes may be located on a rigid body 
which  can  translate  and  rotate  as  the  inflator  moves  during  the  impact.    This 
allows  for  the  point  sources  to  move  in  time.    These  reference  nodes  may  be 
used as the point sources themselves. 
3. 
If  the  *ALE_TANK_TEST  card  is  present,  please  see  the  Remarks  under  that 
card. 
Example: 
Consider a tank test model which consists of the inflator gas (PID 1) and the air inside 
the tank (PID 2).  The 3 load curves define the thermodynamic and kinetic condition of 
the incoming gas.  The nodes define the center of the orifice, and the vector the direction 
of flow at each orifice.
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 
*PART 
inflator gas 
$      PID     SECID       MID     EOSID      HGID      GRAV    ADPOPT      TMID 
         1         1         1         0         0         0         0         0  
*SECTION_POINT_SOURCE 
$    SECID     LCIDT  LCIDVOLR   LCIDVEL NIDLCOOR1 NIDLCOOR2 NIDLCOOR3 
         1         3         4         5         0         0         0 
$   NODEID    VECTID      AREA   
     24485         3    15.066          
       ...      
     24557         3    15.066 
*PART 
air inside the tank 
$      PID     SECID       MID     EOSID      HGID      GRAV    ADPOPT      TMID 
         2         2         2         0         0         0         0         0 
*SECTION_SOLID 
$    SECID    ELFORM       AET 
         2        11         0 
*ALE_MULTI-MATERIAL_GROUP 
$      SID   SIDTYPE 
         1         1 
         2         1 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8
*SECTION_POINT_SOURCE_MIXTURE 
Purpose:    This  command  provides  (a)  an  element  formulation  for  a  solid  ALE  part  of 
the  type  similar  to  ELFORM = 11  of  *SECTION_SOLID,  and  (b)  the  inlet  gas  injection 
boundary condition for multiple-gas mixture in-flow via a set of point source(s).  It also 
provides  the  inflator  orifice  geometry  information.    This  must  be  used  in  combination 
with  the  *MAT_GAS_MIXTURE  and/or  *INITIAL_GAS_MIXTURE  card  . 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SECID 
LCIDT 
Not Used
LCIDVEL 
NIDLC1 
NIDLC2 
NIDLC3 
IDIR 
Type 
I/A 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
I 
0 
8 
Variable 
LCMD1 
LCMD2 
LCMD3 
LCMD4 
LCMD5 
LCMD6 
LCMD7 
LCMD8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Source  Node  Cards.    Include  one  card  for  each  source  node.    This  input  ends  at  the 
next keyword (“*”) card. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NODEID 
VECID 
ORIFA 
Type 
I 
I 
F 
Default 
none 
none 
0.0 
  VARIABLE   
DESCRIPTION
SECID 
Section ID.  A unique number or label must be specified.
LCIDT 
*SECTION_POINT_SOURCE_MIXTURE 
DESCRIPTION
Inflator  gas  mixture  average  stagnation  temperature  load  curve
ID (all gases of the mixture are assumed to have the same average
temperature). 
LCIDVEL 
User-defined inflator gas mixture average velocity load curve ID. 
If  LCIDVEL = 0  or  blank,  LSDYNA  will  estimate  the  inlet  gas
velocity. 
NIDLC001 
The 1st node ID defining a local coordinate . 
NIDLC002 
The 2nd node ID defining a local coordinate . 
NIDLC003 
The 3rd node ID defining a local coordinate . 
IDIR 
A flag for constraining the nodal velocity of the nodes of the ALE
element containing a point source.  If IDIR = 0 (default), then the 
ALE  nodes  behind  the  point  source  (relative  position  of  nodes
based  on  the  vector  direction  of  flow  of  point  source)  will  have
zero  velocity.    If  IDIR = 1,  then  all  ALE  nodes  will  have  velocity 
distributed  based  on  energy  conservation.    The  latter  option
seems to be more robust in airbag modeling . 
LCMD1 
LCMDn 
LCMD8 
The mass flow rate load curve ID of the1st gas in the mixture. 
The mass flow rate load curve ID of the nth gas in the mixture. 
The mass flow rate load curve ID of the 8th gas in the mixture. 
NODEID 
The node ID(s) defining the point sources . 
VECID 
The vector ID defining the direction of flow at each point source. 
ORIFA 
The orifice area at each point source. 
Remarks: 
1.  This  command  is  used  to  define  a  part  that  acts  as  the  ideal  gas  mixture 
injection source.  The associated ALE material (gas mixture) may not be present 
at time zero, but can be introduced (injected) into an existing ALE domain.  For 
airbag application, the input from control volume analysis, inlet mass flow rate, 
𝑚̇ (𝑡), and, inlet stagnation gas temperature, 𝑇̅̅̅̅𝑔𝑎𝑠(𝑡) may be used as direct input 
for ALE analysis.  If available, the user may input a load curve for the gas mix-
ture average inlet velocity.  If not, LS-DYNA will estimate the inlet gas velocity.
2.  The  gas  mixture  is  assumed  to  have  a  uniform  temperature  (𝑇̅̅̅̅ ≈ 𝑇𝑖)  and  inlet 
velocity.    However,  the  species  in  the  mixture  may  each  have  a  different  inlet 
mass flow rate. 
3.  A  brief  review  of  the  concept  used  is  presented.    The  total  energy  (𝑒𝑇)  is  the 
sum of internal (𝑒𝑖) and kinetic (𝑉2
2 ) energies, (per unit mass). 
𝑒𝑇 = 𝑒𝑖 +
𝑉2
𝐶𝑉𝑇𝑠𝑡𝑎𝑔 = 𝐶𝑉𝑇 +
𝑉2
𝑇𝑠𝑡𝑎𝑔 = 𝑇 +
𝑉2
2𝐶𝑉
The distinction between stagnation and static temperatures is shown above.  𝐶𝑉 
is the constant-volume heat capacity.  The gas mixture average internal energy 
per unit mass in terms of mixture species contribution is 
𝜌𝑖
𝜌𝑚𝑖𝑥𝑡𝑢𝑟𝑒
) 𝐶𝑉𝑖𝑇𝑖
= [∑ (
𝜌𝑖
𝜌𝑚𝑖𝑥𝑡𝑢𝑟𝑒
) 𝐶𝑉𝑖
] 𝑇̅̅̅̅
𝑒𝑖 = 𝐶̅𝑉𝑇̅̅̅̅ = ∑ (
𝐶̅𝑉 = [∑ (
𝜌𝑖
𝜌𝑚𝑖𝑥𝑡𝑢𝑟𝑒
) 𝐶𝑉𝑖
]
Since  we  approximate  𝑇̅̅̅̅ ≈ 𝑇𝑖,  then  gas  mixture  average  static  temperature  is 
related to the mixture average internal energy per unit mass as following 
𝑇̅̅̅̅ =
𝑒𝑖
𝜌𝑖
𝜌𝑚𝑖𝑥𝑡𝑢𝑟𝑒
[∑ (
)𝐶𝑉𝑖
]
Note that the “i” subscript under “e” denotes “internal” energy, while the other 
“i”  subscripts  denote  the  “ith”  species  in  the  gas  mixture.    The  total  mixture 
pressure is the sum of the partial pressures of the individual species. 
𝑝̅ = ∑ 𝑝𝑖
The ideal gas EOS applies to each individual species (by default) 
𝑃𝑖 = 𝜌𝑖(𝐶𝑃𝑖 − 𝐶𝑉𝑖)𝑇𝑖 
4.  Generally, it is not possible to conserve both momentum and kinetic (KE) at the 
same  time.    Typically,  internal  energy  (IE)  is  conserved  and  KE  may  not  be.  
This may result in some KE loss (hence, total energy loss).  For many analyses 
this is tolerable, but for airbag application, this may lead to the reduction of the 
inflating potential of the inflator gas. 
In  *MAT_GAS_MIXTURE  computation,  any  kinetic  energy  not  accounted-for 
during advection is stored in the internal energy.  Therefore, there is no kinetic
energy loss, and the total energy of the element is conserved over the advection 
step.    This  is  a  simple,  ad  hoc  approach  that  is  not  rigorously  derived  for  the 
whole system based on first principles.  Therefore it is not guaranteed to apply 
universally to all scenarios.  It is the user’s responsibility to validate the model 
with data. 
5.  Since ideal gas is assumed, there is no need to define the EOS for the gases in 
the mixture. 
6. 
In general, it is best to locate a point source near the center of an ALE element.  
Associated with each point source is an area and a vector indicating flow direc-
tion.    Each  point  source  should  occupy  1  ALE  element  by  itself,  and  there 
should be at least 2 empty ALE elements between any 2 point sources.  A point 
source  should  be  located  at  least  3  elements  away  from  the  free  surface  of  an 
ALE mesh for stability. 
Example 1: 
Consider a tank test model without coupling which consists of: 
-a  background  mesh  with  air  (PID  1 = gas  1)  initially  inside  that  mesh  (tank 
space), and  
-the inflator gas mixture (PID 2 consisting of inflator gases 2, 3, and 4).   
The mixture is represented by one AMMGID and the air by another AMMGID.   
The tank internal space is simply modeled with an Eulerian mesh of the same volume.  
The Tank itself is not modeled thus no coupling is required.  The inflator gases fill up 
this space mixing with the air initially inside the tank. 
The background air (gas 1) is included in the gas mixture definition in this case because 
that air will participate in the mixing process.  Only include in the mixture those gases 
that actually undergo mixing (gases 1, 2, 3 and 4).  Note that for an airbag model, the 
“outside” air should not be included in the mixture (it should be defined independent-
ly)  since  it  does  not  participate  in  the  mixing  inside  the  airbag.    This  is  shown  in  the 
next example. 
The nodes define the center of the orifices, and the vectors define the directions of flow 
at these orifices.
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
*PART 
Tank background mesh, initially filled with air, allows gas mixture to flow in. 
$      PID     SECID       MID     EOSID      HGID      GRAV    ADPOPT      TMID 
         1         1         1         0         0         0         0         0  
*SECTION_SOLID 
$    SECID    ELFORM       AET 
         1        11         0        
$ The next card defines the properties of the gas species in the mixture. 
*MAT_GAS_MIXTURE 
$      MID      
         1        
$      Cv1       Cv2       Cv3       Cv4       Cv5       Cv6       Cv7       Cv8 
    654.47    482.00   2038.30    774.64       0.0       0.0       0.0       0.0 
$      Cp1       Cp2       Cp3       Cp4       Cp5       Cp6       Cp7       Cp8 
    941.32    666.67   2500.00   1071.40       0.0       0.0       0.0       0.0 
$ The next card specifies that gas 1 (background air) occupies PID 1 at time 0. 
*INTIAL_GAS_MIXTURE 
$      SID     STYPE    AMMGID     TEMP0 
         1         1         1    293.00 
$     RHO1      RHO2      RHO3      RHO4      RHO5      RHO6      RHO7      RHO8 
   1.20E-9       0.0       0.0       0.0       0.0       0.0       0.0       0.0 
*PART 
The gas mixture (inlet) definition (no initial mesh required for this PID) 
$      PID     SECID       MID     EOSID      HGID      GRAV    ADPOPT      TMID 
         2         2         1         0         0         0         0         0 
*SECTION_POINT_SOURCE_MIXTURE 
$    SECID     LCIDT   NOTUSED   LCIDVEL NIDLCOOR1 NIDLCOOR2 NIDLCOOR3      IDIR 
         2         1         0         5         0         0         0         0 
$  LCMDOT1   LCMDOT2   LCMDOT3   LCMDOT4   LCMDOT5   LCMDOT6   LCMDOT7   LCMDOT8  
         0         2         3         4         0         0         0         0 
$   NODEID    VECTID      AREA   
     24485         1      25.0          
       ...      
     24557         1      25.0 
*ALE_MULTI-MATERIAL_GROUP 
$      SID   SIDTYPE 
         1         1        
         2         1        
*DEFINE_VECTOR 
$   VECTID     XTAIL     YTAIL     ZTAIL     XHEAD     YHEAD     ZHEAD 
         1       0.0       0.0       0.0       0.0       1.0       0.0   
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
Example 2: 
Consider an airbag inflation model which consists of: 
-a background Eulerian mesh for air initially outside the airbag (PID 1)  
-the inflator gas mixture (PID 2 consisting of inflator gases 1, 2, and 3). 
The mixture is represented by one AMMGID and the air by another AMMGID. 
The background air (PID 1) is NOT included in the gas  mixture definition in this case 
because  that  air  will  NOT  participate  in  the  mixing  process.    Only  include  in  the 
mixture those gases that actually undergo mixing (gases 1, 2, and 3).   Gases 1, 2, and 3 
in  this  example  correspond  to  gases  2,  3,  and  4  in  example  1.    Compare  the  air
properties in PID 1 here to that of example 1.  Note that the *INITIAL_GAS_MIXTURE 
card is not required to initialize the background mesh in this case. 
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 
*PART 
Tank background mesh, initially filled with air, allows gas mixture to flow in. 
$      PID     SECID       MID     EOSID      HGID      GRAV    ADPOPT      TMID 
         1         1         1         0         0         0         0         0 
*SECTION_SOLID 
$    SECID    ELFORM       AET 
         1        11         0        
*MAT_NULL 
$      MID       RHO      PCUT        MU     TEROD     CEROD        YM        PR 
         1   1.20E-9   -1.0E-6       0.0       0.0       0.0        0.0      0.0 
*EOS_IDEAL_GAS 
$    EOSID       CV0       CP0     COEF1     COEF2        T0    RELVOL0 
         1    654.47    941.32       0.0       0.0    293.00        1.0 
$ The next card defines the properties of the gas species in the mixture. 
*PART 
The gas mixture (inlet) definition (no initial mesh required for this PID) 
$      PID     SECID       MID     EOSID      HGID      GRAV    ADPOPT      TMID 
         2         2         2         0         0         0         0         0 
*SECTION_POINT_SOURCE_MIXTURE 
$    SECID     LCIDT   NOTUSED   LCIDVEL NIDLCOOR1 NIDLCOOR2 NIDLCOOR3      IDIR 
         2         1         0         5         0         0         0         0 
$  LCMDOT1   LCMDOT2   LCMDOT3   LCMDOT4   LCMDOT5   LCMDOT6   LCMDOT7   LCMDOT8 
         2         3         4         0         0         0         0         0 
$   NODEID    VECTID      AREA   
     24485         1      25.0          
       ...      
     24557         1      25.0 
*MAT_GAS_MIXTURE 
$      MID      
         2        
$      Cv1       Cv2       Cv3       Cv4       Cv5       Cv6       Cv7       Cv8 
    482.00   2038.30    774.64       0.0       0.0       0.0       0.0 
$      Cp1       Cp2       Cp3       Cp4       Cp5       Cp6       Cp7       Cp8 
    666.67   2500.00   1071.40       0.0       0.0       0.0       0.0 
$ The next card specifies that gas 1 (background air) occupies PID 1 at time 0. 
*ALE_MULTI-MATERIAL_GROUP 
$      SID   SIDTYPE 
         1         1        
         2         1        
*DEFINE_VECTOR 
$   VECTID     XTAIL     YTAIL     ZTAIL     XHEAD     YHEAD     ZHEAD 
         1       0.0       0.0       0.0       0.0       1.0       0.0   
$...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8
*SECTION 
Purpose:  Define section properties for the seat belt elements.  This card is required for 
the *PART Section.  Currently, only the ID is required. 
Seatbelt  Section  Cards.    Include  one  card  for  each  SEATBELT  section.    This  input 
ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SECID 
AREA 
THICK 
Type 
I/A 
F 
F 
Default 
none 
0.01 
none 
  VARIABLE   
DESCRIPTION
Section ID.  A unique number or label must be specified. 
Optional  area  of  cross-section  used  in  the  calculation  of  contact 
stiffness, which is proportional to the cross-section area. 
Optional contact thickness which can be overwritten by a nonzero
SST defined in *CONTACT.  If not defined, a value proportional
to element length is used as the contact thickness. 
SECID 
AREA 
THICK 
Remarks: 
Seatbelt elements are implemented for both explicit and implicit calculations.
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *SECTION_SEATBELT 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Define a seat belt section that is referenced by part 10.  Nothing 
$  more than the sid is required. 
$ 
*SECTION_SEATBELT 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      sid 
       111 
$ 
$ 
*PART 
Seatbelt material 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      pid       sid       mid     eosid      hgid    adpopt 
        10       111       220 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
*SECTION_SHELL_{OPTION} 
Available options include: 
<BLANK> 
EFG 
THERMAL 
XFEM 
Purpose:  Define section properties for shell elements. 
Card  Sets.    For  each  shell  section,  of  a  type  matching  the  keyword’s  options,  include 
one set data cards.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SECID 
ELFORM 
SHRF 
NIP 
PROPT 
QR / IRID 
ICOMP 
SETYP 
Type 
I/A 
I 
F 
Default 
none 
1.0 
Remarks 
  Card 2 
Variable 
1 
T1 
Type 
F 
1 
2 
T2 
F 
3 
T3 
F 
F 
2 
4 
T4 
F 
F 
F 
0.0 
0.0 
I 
0 
I 
1 
5 
6 
7 
8 
NLOC 
MAREA 
IDOF 
EDGSET 
F 
F 
F 
I 
Default 
0.0 
T1 
T1 
T1 
0.0 
0.0 
0.0 
Remarks 
6
Angle Cards.  Additional cards for ICOMP = 1.  Include the minimum number of cards 
necessary  to  input  NIP  values:  8  values  per  card  ⇒  number of cards  =  ceil(NIP 8⁄ )
where ceil(𝑥) = the smallest integer greater than 𝑥. 
  Card 3 
Variable 
1 
B1 
Type 
F 
2 
B2 
F 
3 
B3 
F 
4 
B4 
F 
5 
B5 
F 
6 
B6 
F 
7 
B7 
F 
8 
B8 
F 
EFG Card.  Additional card for EFG keyword option.  See *CONTROL_EFG. 
  Card 4 
Variable 
1 
DX 
2 
3 
4 
5 
6 
7 
8 
DY 
ISPLINE 
IDILA 
IEBT 
IDIM 
Type 
F 
F 
Default 
1.1 
1.1 
I 
0 
I 
0 
I 
I 
-1 or 1 
2 or 1 
Thermal Card.  Additional Card for THERMAL keyword option.  
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ITHELFM 
Type 
Default 
I 
0 
XFEM Card.  Additional card for XFEM keyword option.  See Remark 8.  
  Card 4 
1 
2 
3 
4 
5 
Variable 
CMID 
BASELM  DOMINT 
FAILCR 
PROPCR 
Type 
I 
I 
Default 
36-42 (SECTION) 
I 
I 
0 
I 
1 
7 
8 
LS/FS1 
NC/CL 
6 
FS
User  Defined  Element  Card.    Additional  card  for  ELFORM =  101,102,103,104  or  105. 
See Appendix C 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NIPP 
NXDOF 
IUNF 
IHGF 
ITAJ 
LMC 
NHSV 
ILOC 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
User Defined Element Integration Point Cards.  Additional cards for ELFORM = 101, 
102,  103,  104  or  105.      Define  NIPP  cards  according  to  the  following  format.    See 
Appendix C. 
  Card 6 
Variable 
Type 
1 
XI 
F 
2 
3 
4 
5 
6 
7 
8 
ETA 
WGT 
F 
F 
Default 
none 
none 
none 
User  Defined  Element  Property  Cards.    Include  the  minimum  number  of  cards 
necessary  to  input  LMC  values:  8  values  per  card  ⇒ number of cards  =  ceil(LMC 8⁄ )
where ceil(𝑥) = the smallest integer greater than 𝑥.  See Appendix C. 
  Card 7 
Variable 
Type 
Default 
1 
P1 
F 
0 
2 
P2 
F 
0 
3 
P3 
F 
0 
4 
P4 
F 
0 
5 
P5 
F 
0 
6 
P6 
F 
0 
7 
P7 
F 
0 
8 
P8 
F 
0 
  VARIABLE   
DESCRIPTION
SECID 
Section  ID.    SECID  is  referenced  on  the  *PART  card.    A  unique
VARIABLE   
DESCRIPTION
number or label must be specified. 
ELFORM 
Element formulation options, see Remarks 1 and 2 below: 
EQ.1: 
EQ.2: 
EQ.3: 
EQ.4: 
EQ.5: 
EQ.6: 
EQ.7: 
EQ.8: 
EQ.9: 
EQ.10: 
EQ.11: 
Hughes-Liu, 
Belytschko-Tsay, 
BCIZ triangular shell, 
C0 triangular shell, 
Belytschko-Tsay membrane, 
S/R Hughes-Liu, 
S/R co-rotational Hughes-Liu, 
Belytschko-Leviathan shell, 
Fully integrated Belytschko-Tsay membrane, 
Belytschko-Wong-Chiang, 
Fast (co-rotational) Hughes-Liu, 
EQ.12: 
Plane stress (𝑥-𝑦 plane), 
EQ.13: 
Plane strain (𝑥-𝑦 plane), 
EQ.14:  Axisymmetric solid (𝑥-𝑦 plane, 𝑦-axis of symmetry) -
area weighted , 
EQ.15:  Axisymmetric solid (𝑥-𝑦 plane, 𝑦-axis of symmetry) -
volume weighted, 
EQ.16: 
Fully integrated shell element (very fast), 
EQ.-16:  Fully  integrated  shell  element  modified  for  higher
accuracy, see Remark 0. 
EQ.17: 
EQ.18: 
EQ.20: 
EQ.21: 
EQ.22: 
Fully integrated DKT, triangular shell element, 
Fully  integrated  linear  DK  quadrilateral/triangular
shell   
Fully  integrated  linear  assumed  strain  C0  shell  . 
Fully  integrated  linear  assumed  strain  C0  shell  (5
DOF). 
Linear  shear  panel  element.    3  DOF  per  node.    . 
EQ.23: 
8-node quadratic quadrilateral shell
VARIABLE   
DESCRIPTION
EQ.24: 
EQ.25: 
EQ.26: 
6-node quadratic triangular shell  
Belytschko-Tsay shell with thickness stretch. 
Fully integrated shell with thickness stretch. 
EQ.27:  C0 triangular shell with thickness stretch. 
EQ.29:  Cohesive  shell  element  for  edge-to-edge  connection 
of shells.  See Remark 0. 
EQ.-29:  Cohesive  shell  element  for  edge-to-edge  connection 
of shells (more suitable for pure shear).  See Remark 
0. 
EQ.41:  Mesh-free (EFG) shell local approach.  (more suitable
for crashworthiness analysis) 
EQ.42:  Mesh-free  (EFG)  shell  global  approach. 
suitable for metal forming analysis) 
  (more
EQ.43:  Mesh-free (EFG) plane strain formulation (𝑥-𝑦 plane).
EQ.44:  Mesh-free (EFG) axisymmetric solid formulation (𝑥-𝑦
plane, 𝑦-axis of symmetry). 
EQ.46:  Cohesive  element  for  two-dimensional  plane  strain, 
plane  stress,  and  area-weighted  axisymmetric  prob-
lems (type 14 shells). 
EQ.47:  Cohesive  element  for  two-dimensional  volume-
weighted  axisymmetric  problems  (use  with  type  15
shells). 
EQ.52: 
EQ.54: 
EQ.55: 
Plane strain (𝑥-𝑦 plane) XFEM, base element type 13.
Shell  XFEM,  base  element  type  defined  by  BASELM
(default 16). 
8-node  singular  plane  strain  (𝑥-𝑦  plane)  finite 
element, see Remark 11. 
EQ.98: 
Interpolation shell 
EQ.99: 
Simplified  linear  element  for  time-domain  vibration 
studies.  See Remark 4 below. 
EQ.101:  User defined shell 
EQ.102:  User defined shell 
EQ.103:  User defined shell 
EQ.104:  User defined shell
VARIABLE   
DESCRIPTION
EQ.105:  User defined shell 
EQ.201: 
Isogeometric shells with NURBS. 
See *ELEMENT_SHELL_NURBS_PATCH 
GE.1000:  Generalized 
shell 
element 
formulation 
(user
defined). 
See *DEFINE_ELEMENT_GENERALIZED_SHELL 
The type 18 element is only for linear static and normal modes.  It
can  also  be  used  for  linear  springback  in  sheet  metal  stamping.
For  implicit  modal  computations  element  type  14  must  be
switched to type 15. 
Note  that  the  2D  and  3D  element  types  must  not  be  mixed,  and
different  types  of  2D  elements  must  not  be  used  together.    For
example,  2D  axisymmetric  calculations  can  use  either  element
types  14  or  15  but  these  element  types  must  not  be  mixed
together.    Likewise,  the  plane  strain  element  type  must  not  be 
used  with  either  the  plane  stress  element  or  the  axisymmetric
element types.  In 3D, the different shell elements types, i.e., 1-11 
and 16, can be freely mixed together. 
Shear  correction  factor  which  scales  the  transverse  shear  stress. 
The  shell  formulations  in  LS-DYNA,  with  the  exception  of  the 
BCIZ  and  DK  elements,  are  based  on  a  first  order  shear
deformation  theory  that  yields  constant  transverse  shear  strains
which  violates  the  condition  of  zero  traction  on  the  top  and 
bottom  surfaces  of  the  shell.    The  shear  correction  factor  is
attempt to compensate for this error.  A suggested value is 5/6 for
isotropic  materials.    This  value  is  incorrect  for  sandwich  or
laminated shells; consequently, laminated/sandwich shell theory 
is now an option in some of the constitutive models, e.g., material
types 22, 54, and 55. 
Number  of  through  thickness  integration  points.    Either  Gauss
(default) or Lobatto integration can be used.  The flag for Lobatto
integration  can  be  set  on  the  control  card,  *CONTROL_SHELL. 
The  location  of  the  Gauss  and  Lobatto  integration  points  are
tabulated below. 
EQ.0.0:  set to 2 integration points for shell elements. 
EQ.1.0:  1 point (no bending) 
EQ.2.0:  2 point 
EQ.3.0:  3 point 
SHRF 
NIP
VARIABLE   
DESCRIPTION
EQ.4.0:  4 point 
EQ.5.0:  5 point 
EQ.6.0:  6 point 
EQ.7.0:  7 point 
EQ.8.0:  8 point 
EQ.9.0:  9 point 
EQ.10.:  10 point 
GT.10.:  trapezoidal or user defined rule 
Through  thickness  integration  for  the  two-dimensional  elements 
(options 12-15 above) is not meaningful; consequently, the default
is equal to 1 integration point.  Fully integrated two-dimensional 
elements are available for options 13 and 15 (but not 12 and 14) by 
setting  NIP  equal  to  a  value  of  4  corresponding  to  a  2  by  2
Gaussian  quadrature.    If  NIP  is  0  or  1  and  the  *MAT_SIMPLI-
FIED_JOHNSON_COOK  model 
then  a  resultant
plasticity  formulation  is  activated.    NIP  is  always  set  to  1  if  a 
constitutive model based on resultants is used. 
is  used, 
PROPT 
Printout option (***NOT ACTIVE***): 
EQ.1.0:  average resultants and fiber lengths, 
EQ.2.0:  resultants at plan points and fiber lengths, 
EQ.3.0:  resultants, stresses at all points, fiber lengths. 
QR/IRID 
Quadrature  rule  or  Integration  rule  ID,  see  *INTEGRATION_-
SHELL: 
ICOMP 
LT.0.0:  absolute value is specified rule number, 
EQ.0.0:  Gauss/Lobatto (up to 10 points are permitted), 
EQ.1.0:  trapezoidal, not recommend for accuracy reasons. 
Flag  for  orthotropic/anisotropic  layered  composite  material
model.  This option applies to material types 21, 22, 23, 33, 33_96, 
34, 36, 40, 41-50, 54, 55, 58, 59, 103, 103_P, 104, 108, 116, 122, 133, 
135, 135_PLC, 136, 157, 158, 190, 219, 226, 233, 234, 235, 242, and 
243.    For  these  material  types,  see  *PART_COMPOSITE  as  an 
alternative to *SECTION_SHELL. Note: Please refer to Remark 5
under  *MAT_034  for  additional  information  specific  to  fiber
directions for fabrics.
VARIABLE   
DESCRIPTION
EQ.1:  a  material  angle  in  degrees  is  defined  for  each  through 
thickness  integration  point.    Thus,  each  layer  has  one
integration point. 
SETYP 
Not used (obsolete). 
T1 
T2 
T3 
T4 
NLOC 
MAREA 
Shell thickness at node n1, unless the thickness is defined on the 
*ELEMENT_SHELL_OPTION card. 
Shell thickness at node n2, see comment for T1 above. 
Shell thickness at node n3, see comment for T1 above. 
Shell thickness at node n4, see comment for T1 above. 
Location  of  reference  surface  (shell  mid-thickess)  for  three 
dimensional  shell  elements.    If  nonzero,  the  offset  distance  from
the plane of the nodal points to the reference surface of the shell
in the direction of the shell normal vector is a value, 
offset = −0.50 × NLOC × (average shell thickness). 
Except  for  Mortar  contacts,  this  offset  is  not  considered  in  the 
contact  subroutines  unless  CNTCO  is  set  to  1  in  *CONTROL_-
SHELL.    Alternatively,  the  offset  can  be  specified  by  using  the
OFFSET  option  in  the  *ELEMENT_SHELL  input  section.    For 
Mortar contacts, NLOC or OFFSET determines the location of the 
contact surface regardless the value of CNTCO. 
EQ.1.0:  nodes are located at top surface of shell, 
EQ.0.0:  nodes are located at mid-thickness of shell (default), 
EQ.-1.0: nodes are located at bottom surface of shell. 
Non-structural mass per unit area.  This is additional mass which
comes from materials such as carpeting.  This mass is not directly
included  in  the  time  step  calculation.    Another  and  often  more
convenient  alternative  for  defining  distributed  mass  is  by  the
option:  *ELEMENT_MASS_PART,  which  allows  additional  non-
structural mass to be distributed by an area weighted distribution
to all nodes of a given part ID). 
IDOF 
Treatment of through thickess strain. 
LT.0:  Same as IDOF.EQ.3 but the contact pressure is averaged
over  a  time  –IDOF  in  order  to  reduce  noise  and  thus
VARIABLE   
DESCRIPTION
improve stability. 
EQ.1:  The  thickness  field  is  continuous  across  the  element
edges for metalforming applications.  This option applies
to element types 25 and 26. 
EQ.2:  The  thickness  field  is  discontinuous  across  the  element 
edges.  This is necessary for crashworthiness simulations
due  to  shell  intersections,  sharp  included  angles,  and
non-smooth  deformations.    This  option  applies  to  ele-
ment  types  25,  26  and  27  and  is  mandatory  for  element
27.  This is the default for these element types. 
EQ.3:  The  thickness  strain  is  governed  by  the  contact  stress,
meaning that the strain is adjusted for the through thick-
ness  stress  to  equilibrate  the  contact  pressure.    This  op-
tion applies to element types 2, 4, and ±16 . 
Edge node set required for shell type seatbelts.  Input an ordered
set  of  nodes  along  one  of  the  transverse  edges  of  a  seatbelt.      If
there is no retractor associated with a belt, the node set can be on
either  edge.    If  the  retractor  exists,  the  edge  must  be  on  the 
retractor  side  and  input  in  the  same  sequence  of  retractor  node
set.    Therefore,  another  restriction  on  the  seatbelt  usage  is  that
each  belt  has  its  own  section  definition  and,  therefore,  a  unique
part  ID.    See  Figure  17-16  in  the  section  *ELEMENT_SEATBELT 
for additional clarification. 
𝛽1, material angle at first integration point 
𝛽2, material angle at second integration point 
𝛽3, material angle at third integration point 
⋮  
𝛽nip, material angle at NIPthintegration point. 
Normalized dilation parameters of the kernel function in X and Y
directions.    The  normalized  dilation  parameters  of  the  kernel
function  are  introduced  to  provide  the  smoothness  and  compact
support  properties  on  the  construction  of  the  mesh-free  shape 
functions.  Values between 1.0 and 2.0 are recommended.  Values
smaller than 1.0 are not allowed.  Larger values will increase the
computation  time  and  will  sometimes  result  in  a  divergence
problem. 
EDGSET 
B1 
B2 
B3 
⋮ 
BNIP 
DX, DY
ISPLINE 
*SECTION_SHELL 
DESCRIPTION
Replace  the  choice  for  the  EFG  kernel  functions  definition  in 
*CONTROL_EFG.  This allows  users to define different ISPLINE 
in different sections. 
IDILA 
Replace  the  choice  for  the  normalized  dilation  parameter
definition  in  *CONTROL_EFG.    This  allows  users  to  define 
different IDILA in different sections. 
IEBT 
Essential boundary condition treatment 
EQ.1:  Full transformation (default for ELFORM = 42) 
EQ.-1:  Without full transformation (default for ELFORM = 41)
EQ.3:  Coupled FEM/EFG  
EQ.7:  Maximum entropy approximation 
IDIM 
For mesh-free shell local approach (ELFORM = 41) 
EQ.1:  First-kind local boundary condition method 
EQ.2:  Gauss integration (default) 
For mesh-free shell global approach (ELFORM = 42) 
EQ.1:  First-kind local boundary condition method (default) 
EQ.2:  Second-kind local boundary condition method 
ITHELFM 
Thermal shell formulation 
EQ.0:  Default is governed by THSHEL on *CONTROL_SHELL
EQ.1:  Thick thermal shell 
EQ.2:  Thin thermal shell 
CMID 
Cohesive material ID (only *MAT_COHESIVE_TH is available) 
BASELM 
Base  element  type  for  XFEM  (type  13  for  2D,  types  2  and  16  for 
shell) 
DOMINT 
Option for domain integration in XFEM: 
EQ.0:  Phantom element integration 
EQ.1:  Subdomain  integration  with  triangular  local  boundary
integration (available in 2D only) 
FAILCR 
Option for different failure criteria:
VARIABLE   
DESCRIPTION
EQ.1:  Maximum tensile stress 
EQ.2:  Maximum shear stress 
EQ.-1: Effective plastic strain  
EQ.-2: Crack length dependent EPS  
EQ.-n:  n > 10,  (n-10)  points  to  HSVS  for  mat282/283   
PROPCR 
Not used 
FS 
LS 
NC 
FS 
FS1 
CL 
NIPP 
Failure strain/Failure critical value 
Length scale for strain regularization. > 0 activates regularization, 
available for FAILCR = -1 and –n for mat282/283 
Number of cracks allowed in the part 
When FAILCR = -2, following three parameters represent : 
Initial failure plastic strain 
Final failure plastic strain 
Crack length failure strain reaches FS1 
Number of in-plane integration points for user-defined shell (0 if 
resultant/discrete element) 
NXDOF 
Number  of  extra  degrees  of  freedom  per  node  for  user-defined 
shell 
IUNF 
Flag for using nodal fiber vectors in user-defined shell: 
EQ.0:  Nodal fiber vectors are not used. 
EQ.1:  Nodal fiber vectors are used. 
IHGF 
Flag for using hourglass stabilization (NIPP.GT.0) 
EQ.0:  Hourglass stabilization is not used 
EQ.1:  LS-DYNA hourglass stabilization is used
VARIABLE   
DESCRIPTION
EQ.2:  User-defined hourglass stabilization is used 
EQ.3:  Same as 2, but the resultant material tangent moduli are
passed 
ITAJ 
Flag for setting up finite element matrices (NIPP.GT.0) 
EQ.0:  Set up matrices wrt isoparametric domain 
EQ.1:  Set up matrices wrt physical domain 
LMC 
Number of property parameters 
NHSV 
Number of history variables 
ILOC 
Coordinate system option: 
EQ.0:  Pass all variables in LS-DYNA local coordinate system 
EQ.1:  Pass all variables in global coordinate system 
XI 
ETA 
WGT 
P1 
P2 
⋮ 
First isoparametric coordinate 
Second isoparametric coordinate 
Isoparametric weight 
First user defined element property. 
Second user defined element property. 
⋮  
PLCM 
LCMth user defined element property.
Gaussian Quadrature Points 
Point 
1 Point 
2 Points 
3 Points 
4 Points 
5 Points 
#1 
#2 
#3 
#4 
#5 
 .0 
-.5773503  .0 
-.8611363   .0 
+.5773503 -.7745967 -.3399810  -.9061798 
+.7745967 +.3399810  -.5384693 
+.8622363  +.5384693 
+.9061798 
Point 
6 Points 
7 Points 
8 Points 
9 Points 
10 Points 
#1 
#2 
#3 
#4 
#5 
#6 
#7 
#8 
#9 
#10 
-.9324695  -.9491080 -.9702896 -.9681602  -.9739066 
-.6612094  -.7415312 -.7966665 -.8360311  -.8650634 
-.2386192  -.4058452 -.5255324 -.6133714  -.6794096 
+.2386192   .0 
-.1834346 -.3242534  -.4333954 
+.6612094  +.4058452 +.1834346  .0 
-.1488743 
+.9324695  +.7415312 +.5255324 +.3242534  +.1488743 
+.9491080 +.7966665 +.6133714  +.4333954 
+.9702896 +.8360311  +.6794096 
+.9681602  +.8650634 
+.9739066 
Location of through thickness Gauss integration points.  The coordinate is referenced 
to  the  shell  midsurface  at  location  0.    The  inner  surface  of  the  shell  is  at  -1  and  the 
outer surface is at +1.
Lobatto Quadrature Points 
Point 
1 Point 
2 Points 
3 Points 
4 Points 
5 Points 
#1 
#2 
#3 
#4 
#5 
 0.0 
-1.0 
+1.0 
-1.0 
 0.0 
-0.4472136 -1.0 
+0.4472136 -0.6546537
+1.0 
+0.6546537
+1.0 
Point 
6 Points 
7 Points 
8 Points 
9 Points 
10 Points 
#1 
#2 
#3 
#4 
#5 
#6 
#7 
#8 
#9 
#10 
-1.0 
-1.0
-1.0
-1.0
-1.0
-0.7650553 -0.8302239 -0.8717401 -0.8997580 -0.9195339
-0.2852315 -0.4688488 -0.5917002 -0.6771863 -0.7387739
+0.2852315  0.0
-0.2092992 -0.3631175 -0.4779249
+0.7650553 +0.4688488 +0.2092992 0.0
-0.1652790
+1.0 
+0.8302239 +0.5917002 +0.3631175 +0.1652790
+1.0
+0.8717401 +0.6771863 +0.4779249
+1.0
+0.8997580 +0.7387739
+1.0
+0.9195339
+1.0
Location of through thickness Lobatto integration points.  The coordinate is referenced 
to the shell midsurface at location 0.  The inner surface of the shell is at -1 and the outer 
surface is at +1. 
Remarks: 
1.  Formulation.  The default shell formulation is 2 unless overridden by THEORY 
in *CONTROL_SHELL.  ELFORM in *SECTION_SHELL overrides THEORY. 
For  implicit  calculations  the  following  element  formulations  are  implemented: 
2, 5, 6, 10, 12,12, 13, 14, 15, 16, -16, 17, 18, 20, 21, 22, 23, 24, 25, 26, 27, 29, 41, 42, 
55.  
If another element formulation is requested for an implicit analysis, LS-DYNA 
will substitute one of the above in place of the one chosen. 
2.  Linear Elements Type 18 and 20.  The linear elements consist of an assembly 
of membrane and plate elements.  They have six degrees of freedom per node 
and  can,  therefore,  be  connected  to  beams,  or  used  in  complex  shell  surface
intersections.    These  elements  possess  the  required  zero  energy  rigid  body 
modes  and  have  exact  constant  strain  and  curvature  representation,  i.e.    they 
pass  all  the  first  order  patch  tests.    In  addition,  the  elements  have  behavior 
approaching linear bending (cubic displacement) in the plate-bending configu-
ration. 
a)  The  membrane  component  is  based  on  an  8-node/6-node  isoparametric 
mother  element  which  incorporates  nodal  in-plane  rotations  through  cu-
bic displacement constraints of the sides [Taylor 1987; Wilson 2000]. 
b)  The  plate  component  of  element  18  is  based  on  the  Discrete  Kirchhoff 
Quadrilateral  (DKQ)  [Batoz  1982].    Because  the  Kirchhoff  assumption  is 
enforced, the DKQ is transverse-shear rigid and can only be used for thin 
shells.  No transverse shear stress information is available.  The triangle is 
based  on  a  degeneration  of  the  DKQ.    This  element  sometimes  gives 
slightly lower eigenvalues when compared with element type 20. 
c)  The plate component of element 20 is based on the 8-node serendipity el-
ement.    At  the  mid-side,  the  parallel  rotations  and  transverse  displace-
ments  are  constrained  and  the  normal rotations  are  condensed  to yield  a 
4-node element.  The element is based on thick plate theory and is recom-
mended for thick and thin plates. 
d)  The quadrilateral elements contain a warpage correction using rigid links. 
e)  The membrane component of element 18 has a zero energy mode associat-
ed with in-plane rotations.  This is automatically suppressed in a non-flat 
shell by the plate stiffness of the adjacent elements.  In contrast, element 20 
has no spurious zero energy modes. 
3.  Linear Shear Element (22).  The linear shear panel element resist tangential in 
plane shearing along the four edges and can only be used with the elastic mate-
rial constants of *MAT_ELASTIC.  Membrane forces and out-of-plane loads are 
not resisted. 
4.  Simplified  Element  for  Time  Domain  Vibrations  (99).    Element  type  99  is 
intended  for  vibration  studies  carried  out  in  the  time  domain.    These  models 
may  have  very  large  numbers  of  elements  and  may  be  run  for  relatively  long 
durations.  The purpose of this element is to achieve substantial CPU savings.  
This  is  achieved  by  imposing  strict  limitations  on  the  range  of  applicability, 
thereby simplifying the calculations:  
a)  Elements  must  be  rectangular;  all  edges  must  parallel  to the  global  𝑥-,  𝑦- 
or 𝑧-axis; 
b)  Small displacement, small strain, negligible rigid body rotation;
*SECTION_SHELL 
If these conditions are satisfied, the performance of the element is similar to the 
fully integrated shell (ELFORM = 16) but at less CPU cost than the default Be-
lytschko-Tsay shell element (ELFORM = 2).  Single element torsion and in-plane 
bending modes are included; meshing guidelines are the same as for fully inte-
grated shell elements. 
No damping is included in the element formulation (e.g.  volumetric damping).  
It is strongly recommended that damping be applied, e.g.  *DAMPING_PART_-
MASS or *DAMPING_FREQUENCY_RANGE. 
5.  2D  Formulations.    For  2D  formulations  (12-15,  46,  47),  nodes  must  lie  in  the 
global 𝑥-𝑦 plane, i.e., the 𝑧-coordinate must be zero.  Furthermore, the element 
normal  should  be  in  positive  𝑧  direction.    For  axisymmetric  element  formula-
tions, the global 𝑦-axis is taken as the axis of symmetry and all nodes must have 
𝑥-coordinate values greater than or equal to 0. 
Shell  thickness  values  on  Card  2  are  ignored  by  formulations  13,  14,  and  15.   
For  formulation  14  Input  values  of  loads,  lumped  masses,  discrete  element 
stiffnesses,  etc.    in  axisymmetric  models  are  interpreted  as  values per  unit  cir-
cumference  (i.e.,  per  unit  length  in  the  circumferential  direction)  whereas  for 
formulation  15  they  are  interpreted  per  radian.    Output  of  forces  for  shell  for-
mulation 15 are in units of force per radian, e.g, as in bndout, nodfor, secforc, 
spcforc, rcforc.  The units of forces output for shell formulation 14 are, at pre-
sent, inconsistent.  For defining contact in 2D simulations, see the entry for the 
*CONTACT_2D keyword. 
6.  Shells  with  Thickness  Stretch.    Shell  element  formulation  25  and  26  are  the 
fully  integrated  shell  element  based  on  the  Belytschko-Tsay  element  but  with 
two  additional  degrees  of  freedom  allowing  for  a  linear  variation  of  strain 
through  the  thickness.    By  default,  the  thickness  field  is  continuous  across  the 
element  edges  implying  that  there  can  be  no  complex  intersections  since  this 
would lock up the structure.  It assumes a relatively flat surface and is intended 
primarily  for  sheets  in  metal  forming.    By  specifying  IDOF = 2,  the  thickness 
field is decoupled between elements which makes the element suited for crash.  
If there are any thickness stretch triangles (formulation 27), IDOF must be set to 
2. 
7.  Seatbelts.  Users must input a set of nodes along one of the transverse edges of 
a seatbelt.  If there is no retractor associated with a belt, the node set can be on 
either edge.  If the retractor exists, the edge should be on the retractor side and 
input in the same sequence of retractor node set.  Therefore, another restriction 
on the seatbelt usage is each belt has its own section definition and a different 
part.
8.  Fracture.    XFEM  2D  and  shell  formulations  are  recommended  for  brittle  or 
semi-brittle fracture with pre-cracks, see *BOUNDARY_PRECRACK, or geome-
try imperfection such as a notch or a hole.  XFEM shell formulation can be used 
for ductile fracture analysis with regularized effective plastic strain criterion. 
9.  Discrete  Kirchoff  Theory  Shell  (17).    Shell  element  formulation  17  (DKT)  is 
based on discrete Kirchhoff theory.  It neglects out-of-plane shear strain energy 
and  is  thus  valid  only  for  thin  plates  where  shear  strain  energy  is  negligible 
compared to bending energy. 
10.  Limitations of Area-Weight Shell (14).  The exact stiffness matrix for the area-
weighted shell formulation type 14 is nonsymmetric.  The nonsymmetric terms 
are  dropped  for  computational  efficiency,  making  this  formulation  unsuitable 
for implicit linear analysis and eigenvalue analysis.   It may, however, be used 
effectively for implicit nonlinear analysis. 
For  explicit  dynamics,  viscous  hourglass  limits  high  frequency  noise  that  may 
otherwise lead to nonphysical element distortion when nodes are on or near the 
axis  of  symmetry.    Viscosity  can  be  added  to  type  6  or  7  hourglass  control  by 
using VDC > 0 under the *HOURGLASS keyword.  Alternatively, type 1 hour-
glass control is viscous. 
11.  Eight Node Singular Shell (55).  The eight-noded singular element for fracture 
analysis is based on the eight-noded quadratic quadrilateral element.  There are 
two ways to include the singularity around the crack tip: 
a)  Move  the  two  mid-nodes  on  the  edges  connected  to  the  crack  tip  to  the 
quarter location and obtain a strain singularity of 1/√𝑟  
b)  Collapse  the  three  nodes  on  one  side  of  a  quadrilateral  element  to  the 
crack  tip  (but  the  three  nodes  remain  independent)  and  move  the  two 
neighboring mid-nodes to the quarter location to obtain a strain singulari-
ty of 1/𝑟. 
This element uses 3×3 quadrature and is available to both implicit and explicit 
analyses. 
Cohesive  Shell  (29).    Element  type  +/-29  is  a  cohesive  element  that  models 
cohesive  interfaces  between  shell  element  edges.    The  element  takes  bending 
forces into account and uses drilling force stabilization. 
Consider  two  shell  elements  in  the  same  plane  with  nodes 𝑚1, 𝑚2,  𝑚3,  𝑚4, 𝑛1, 
𝑛2,  𝑛3,  and  𝑛4  such  that  the (𝑚3, 𝑚4)  edge  and  the (𝑛1, 𝑛2)  edge  are  connected 
through a cohesive shell having nodes 𝑚4, 𝑚3, 𝑛2, and 𝑛1, see Figure 36-23.  The 
initial  area  of  the  cohesive  element  may  be  zero,  in  which  case  density  is  de-
fined in terms of the length of the single connecting edge.
Element  type  +/-29  works  similarly  to  solid  element  type  20.    For  example, 
extruding  the  two  non-cohesive  shells  in  their  respective  normal  directions 
defines  two  8  node  solids.    The  cohesive  mid-surface  is  located  between  the 
opposing  faces  of  the  solids,  and  tractions  are  calculated  in  four  mid-surface 
points  using  differences  of  displacements  between  the  opposing  faces,  giving 
rise to nodal forces and moments in the cohesive shell nodes 𝑚4, 𝑚3, 𝑛2, and 𝑛1.  
Additional details can be found in the Theory Manual. 
Difference between type 29 and -29: In both formulations, the cohesive coordi-
nate system direction 𝑞2 is defined by the midpoints of the (𝑛1, 𝑚4) and (𝑛2, 𝑚3) 
edges.  Type 29 defines the cohesive midsurface normal 𝑞3 using the midpoints 
on  the  far  side  edges (𝑚1, 𝑚2)  and  (𝑛3, 𝑛4),  while  type  -29  defines  𝑞1  to  be the 
mean  of  the  neighboring  element  normals.    Thus,  in  pure  out-of-plane  shear, 
type 29 will initially have pure tangential traction that turns into a normal trac-
tion  as  the  separation  increases,  while  type  -29  will  only  have  tangential  trac-
tion. 
𝒒3
𝑛4
𝑛1
𝑚4
𝑚1
𝒒1 
𝑛3
𝑛2
𝑚3
𝑚2
𝒒2
  Figure [36-23].  Cohesive interface coordinate system for element type +/-29
12.  Accurate fully-integrated shell (-16).  Accuracy issues have been observed in 
shell formulation 16 under large deformations/rotations over a single time step.  
Formulation  -16  is  a  correspondently  enhanced  version  of  formulation  16.  
Formulation  16  is  unchanged  to  maintain  back  compatibility  and,  although, 
element  -16  is  supported  in  explicit  mode  it  is  primarily  intended  for  implicit 
time  integration.    A  strongly  objective  version  can  be  activated  by  combining 
ELFORM = -16  and  IACC = 1  on  *CONTROL_ACCURACY,  thereby  ensuring 
that arbitrarily large rigid body rotation in a single step will transform stresses 
correctly and not generate any spurious strains.
13.  XFEM  ductile  fracture.  This  feature  is  supported  by  a  joint  research  among 
Honda,  JSOL  and  LSTC.    For  FAILCR = -2,  the  failure  strain  is  defined  by: 
EPS = FS+(FS1-FS)*min(L/CL, 1.0) where L is the current crack length. 
Example: 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *SECTION_SHELL 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  Define a shell section that specifies the following: 
$     elform = 10  Belytschko-Wong-Chiang shell element formulation. 
$        nip = 3   Three through the shell thickness integration points. 
$    t1 - t4 = 2.0 A shell thickness of 2 mm at all nodes. 
$ 
*SECTION_SHELL 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      sid    elform      shrf       nip     propt   qr/irid     icomp 
         1        10              3.0000 
$ 
$       t1        t2        t3        t4      nloc 
       2.0       2.0       2.0       2.0 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
*SECTION_SOLID_{OPTION} 
Available options include: 
<BLANK> 
EFG 
SPG 
Purpose:  Define section properties for solid continuum and fluid elements. 
Card  Sets.    For  each  unique  solid  section,  include  one  set  of  data  cards.    The  EFG 
option and the SPG option cannot both appear in the same model.  This input ends at 
the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SECID 
ELFORM 
AET 
Type 
I/A 
I 
I 
EFG Card.  Additional card for the EFG keyword option.  See *CONTROL_EFG. 
3 
4 
5 
6 
7 
8 
DZ 
ISPLINE 
IDILA 
IEBT 
IDIM 
TOLDEF 
  Card 2 
Variable 
1 
DX 
Type 
F 
2 
DY 
F 
Default 
1.01 
1.01 
1.01 
F 
I 
0 
I 
0 
I 
1 
I 
2 
F 
0.01
Optional EFG Card.  Additional optional card for the EFG keyword option.  See *CON-
TROL_EFG. 
  Card 3 
1 
2 
3 
Variable 
IPS 
STIME 
IKEN 
Type 
Default 
I 
0 
F 
1020 
I 
0 
4 
SF 
I 
0.0 
5 
6 
CMID 
IBR 
I 
I 
1 
7 
DS 
F 
8 
ECUT 
F 
1.01 
0.1 
SPG Card.  Additional card for the SPG keyword option.  
3 
4 
5 
6 
7 
8 
DZ 
ISPLINE 
KERNEL 
LSCALE 
SMSTEP  SWTIME 
  Card 2 
Variable 
1 
DX 
Type 
F 
2 
DY 
F 
Default 
1.50 
1.50 
1.50 
F 
I 
0 
I 
0 
F 
I 
F 
15 
Optional SPG Card.  Additional optional card for the SPG keyword option. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IDAM 
FS 
STRETCH
ITB 
Type 
Default 
I 
0 
F 
F 
I
User Defined Element Card.  Additional card for ELFORM = 101, 102, 103, 104 or 105. 
See Appendix C. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NIP 
NXDOF 
IHGF 
ITAJ 
LMC 
NHSV 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
Integration Point Card.  Additional card for ELFORM = 101, 102, 103, 104 or 105.  Add 
NIP cards adhering to the format below.  Because the default value for NIP is 0, these 
cards are read only for user-defined elements.  See Appendix C. 
Card 
Variable 
Type 
1 
XI 
F 
2 
3 
4 
5 
6 
7 
8 
ETA 
ZETA 
WGT 
F 
F 
F 
Default 
none 
none 
none 
none 
Property Parameter Cards.  Additional card for ELFORM = 101, 102, 103, 104 or 105. 
Add LMC property parameters by packing 8 parameters per card.  See Appendix C. 
Card 
Variable 
Type 
Default 
1 
P1 
F 
0 
2 
P2 
F 
0 
3 
P3 
F 
0 
4 
P4 
F 
0 
5 
P5 
F 
0 
6 
P6 
F 
0 
7 
P7 
F 
0 
8 
P8 
F 
0 
  VARIABLE   
SECID 
DESCRIPTION
Section  ID.    SECID  is  referenced  on  the  *PART  card.    A  unique
number or label must be specified. 
ELFORM 
Element formulation options.  Remark 2 enumerates the element
VARIABLE   
DESCRIPTION
formulations available for implicit calculations: 
EQ.-2: 
EQ.-1: 
EQ.0: 
EQ.1: 
EQ.2: 
EQ.3: 
EQ.4: 
EQ.5: 
EQ.6: 
EQ.7: 
EQ.8: 
EQ.9: 
EQ.10: 
EQ.11: 
EQ.12: 
EQ.13: 
Fully  integrated  S/R  solid  intended  for  elements
with poor aspect ratio, accurate formulation  
Fully  integrated  S/R  solid  intended  for  elements
with  poor  aspect  ratio,  efficient  formulation   
1  point  corotational  for  *MAT_MODIFIED_HONEY-
COMB  
Constant  stress  solid  element:  default  element  type.
By  specifying  hourglass  type  10  with  this  element,  a
Cosserat  Point    Element  is  invoked,  see  *CON-
TROL_HOURGLASS 
Fully integrated S/R solid  
Fully integrated quadratic 8 node element with nodal 
rotations 
S/R  quadratic  tetrahedron  element  with  nodal
rotations 
1 point ALE 
1 point Eulerian 
1 point Eulerian ambient 
Acoustic 
1  point  corotational  for  *MAT_MODIFIED_HONEY-
COMB  
1 point tetrahedron  
1 point ALE multi-material element 
1 point integration with single material and void 
1 point nodal pressure tetrahedron  
EQ.14: 
8 point acoustic 
EQ.15: 
EQ.16: 
2 point pentahedron element  
4  or  5  point  10-noded  tetrahedron  . 
By  specifying  hourglass  type  10  with  this  element,  a
Cosserat Point Element is invoked, see *CONTROL_-
HOURGLASS
VARIABLE   
DESCRIPTION
EQ.17: 
EQ.18: 
EQ.19: 
EQ.20: 
EQ.21: 
EQ.22: 
10-noded composite tetrahedron  
8  point  enhanced  strain  solid  element  for  linear
statics only  
8-noded,  4  point  cohesive  element   
8-noded,  4  point  cohesive  element  with  offsets  for
use with shells  
6-noded,  1  point  pentahedron  cohesive  element   
6-noded, 1 point pentahedron cohesive element with
offsets for use with shells  
EQ.23: 
20-node solid formulation 
EQ.24: 
27-noded,  fully 
element 
integrated  S/R  quadratic  solid
EQ.41:  Mesh-free (EFG) solid formulation  
EQ.42:  Adaptive 4-noded mesh-free (EFG) solid formulation 
 
EQ.43:  Mesh-free enriched finite element 
EQ.45:  Tied Mesh-free enriched finite element 
EQ.47: 
Smoothed particle Galerkin method 
EQ.98: 
Interpolation solid 
EQ.99: 
Simplified  linear  element  for  time-domain  vibration 
studies  
EQ.101:  User defined solid 
EQ.102:  User defined solid 
EQ.103:  User defined solid 
EQ.104:  User defined solid 
EQ.105:  User defined solid 
EQ.115:  1 point pentahedron element with hourglass control 
GE.201:  Isogeometric solids with NURBS.   
GE.1000:  Generalized  user-defined  solid  element  formulation
VARIABLE   
DESCRIPTION
AET 
Ambient Element type:  Can be defined for ELFORM 7, 11 and 12.
EQ.0: Non-ambient 
EQ.1: Temperature (not currently available) 
EQ.2: Pressure and temperature (not currently available) 
EQ.3: Pressure outflow (obsolete) 
EQ.4: Pressure inflow/outflow (Default for ELFORM 7) 
EQ.5: Receptor 
for  blast 
load 
 
Normalized dilation parameters of the kernel function in 𝑥, 𝑦 and 
𝑧  directions.    The  normalized  dilation  parameters  of  the  kernel
function  are  introduced  to  provide  the  smoothness  and  compact
support  properties  on  the  construction  of  the  mesh-free  shape 
functions.  Values between 1.0 and 1.5 are recommended.  Values 
smaller than 1.0 are not allowed.  Larger values will increase the
computation  time  and  will  sometimes  result  in  a  divergence
problem. 
DX, DY, DZ 
ISPLINE 
Replace  the  choice  for  the  EFG  kernel  functions  definition  in
*CONTROL_EFG.  This allows  users to define different ISPLINE 
in different sections. 
EQ.0: Cubic spline function (default). 
EQ.1: Quadratic spline function. 
EQ.2: Cubic spline function with circular shape. 
IDILA 
Replace  the  choice  for  the  normalized  dilation  parameter 
definition  in  *CONTROL_EFG.    This  allows  users  to  define 
different IDILA in different sections. 
EQ.0: Maximum distance based on the background elements. 
EQ.1: Maximum distance based on surrounding nodes. 
IEBT 
Essential boundary condition treatment: See Remark 9 and 10. 
EQ.1:  Full transformation method (default) 
EQ.-1: (w/o transformation) 
EQ.2:  Mixed transformation method 
EQ.3:  Coupled FEM/EFG method
VARIABLE   
DESCRIPTION
EQ.4:  Fast transformation method 
EQ.-4: (w/o transformation) 
EQ.5:  Fluid  particle  method  for  E.O.S  and  *MAT_ELASTIC_-
FLUID  materials,  currently  supports  only  4-noded 
background elements. 
EQ.7:  Maximum entropy approximation 
IDIM 
Domain integration method: See Remark 11. 
EQ.1:  Local boundary integration 
EQ.2:  Two-point Gauss integration (default) 
EQ.3:  Improved Gauss integration for IEBT = 4 or -4 
EQ.-1: Stabilized  EFG  integration  method  (apply  to  6-noded 
cell, 8-noded cell or combination of these two) 
EQ.-2: EFG  fracture  method  (apply  to  4-noded  cell  and  SMP 
only) 
TOLDEF 
Deformation  tolerance  for  the  activation  of  adaptive  EFG  Semi-
Lagrangian and Eulerian kernel. See Remark 12. 
EQ.0.0: Lagrangian kernel 
GT.0.0:  Semi_Lagrangian kernel 
LT.0.0:  Eulerian kernel 
IPS 
EQ.0: No pressure smoothing (default) 
EQ.1: Moving-least squared pressure recovery 
STIME 
Time to switch from stabilized EFG to standard EFG formulation 
IKEN 
EQ.0: Moving-least-square  approximation 
(default,  recom-
mended) 
EQ.1: Maximum Entropy approximation 
SF 
CMID 
Failure  strain,  recommended  as  an  extra  condition  for  the  crack
initiation  under  slow  loading  besides  the  stress-based  cohesive 
law 
Cohesive material ID for EFG fracture analysis (only Mode I crack
is considered and only *MAT_COHESIVE_TH is available)
VARIABLE   
DESCRIPTION
IBR 
DS 
ECUT 
EQ.1: No branching allowed 
EQ.2: Branching is allowed 
Normalized  support  defined  for  computing  the  displacement
jump in fracture analysis 
Define the minimum distance to the node that a crack surface can
cut to the edge 
KERNEL 
Type of kernel approximation 
EQ.0: updated  Lagrangian  kernel,  no  failure, 
less  shear
deformation 
EQ.1: Eulerian  kernel, 
deformation 
failure  analysis,  global  extreme
EQ.2: Semi-pseudo  Lagrangian  kernel,  failure  analysis,  local 
extreme deformation 
LSCALE 
Length scale for displacement regularization (not used yet) 
SMSTEP 
Interval of time steps to conduct displacement regularization 
SWTIME 
Time  to  switch  from  updated  Lagrangian  kernel  to  Eulerian
kernel 
IDAM 
Option of damage mechanism  
EQ.0: Continuum damage mechanics (default), the failed nodes 
are not eroded but converted to free nodes still carrying
mass and momentum 
EQ.1: Phenomenological strain damage 
FS 
Failure effective plastic strain if IDAM = 1 
STRETCH 
Stretching parameter if IDAM = 1 
ITB 
Flag for using stabilization 
EQ.0:  standard  meshfree  approximation  +  T-bond 
algorithm 
EQ.1:  fluid particle approximation (accurate but slow) 
EQ.2:  simplified  fluid  particle  approximation  (efficient  and
robust) 
failure
NIP 
*SECTION_SOLID 
DESCRIPTION
Number of integration points for user-defined solid (0 if resultant 
element) 
NXDOF 
Number  of  extra  degrees  of  freedom  per  node  for  user-defined 
solid 
IHGF 
Flag for using hourglass stabilization (NIP.GT.0) 
EQ.0: Hourglass stabilization is not used 
EQ.1: LS-DYNA hourglass stabilization is used 
EQ.2: User-defined hourglass stabilization is used 
EQ.3: Same as 2, but the resultant material tangent moduli are
passed 
ITAJ 
Flag for setting up finite element matrices (NIP.GT.0) 
EQ.0: Set up matrices wrt isoparametric domain 
EQ.1: Set up matrices wrt physical domain 
LMC 
Number of property parameters 
NHSV 
Number of history variables 
XI 
ETA 
ZETA 
WGT 
First isoparametric coordinate 
Second isoparametric coordinate 
Third isoparametric coordinate 
Isoparametric weight 
PI 
Ith property parameter 
Remarks: 
1.  ESORT  to  Stabilize  Degenerate  Solids.    The  ESORT  variable  of  the  *CON-
TROL_SOLID keyword can be set to automatically convert degenerate tetrahe-
into  more  suitable  solid  element 
drons  and  degenerate  pentahedrons 
formulations.    The  sorting  is  performed  internally  and  is  transparent  to  the 
user.  See *CONTROL_SOLID for details.
2. 
Implicit  Analysis.    For  implicit  calculations  the  following  element  choices  are 
implemented: 
EQ.-2:  Fully  integrated  S/R  solid  element  for  poor  aspect  ratios,  ac-
curate formulation. 
EQ.-1:  Fully integrated S/R solid element for poor aspect ratios, effi-
cient formulation. 
EQ.1:  Constant stress solid element. 
EQ.2:  Fully integrated S/R solid. 
EQ.3:  Fully integrated 8 node solid with rotational DOFs. 
EQ.4:  Fully integrated S/R 4 node tetrahedron with rotational DOFs. 
EQ.10:  1 point tetrahedron. 
EQ.13:  1 point nodal pressure tetrahedron. 
EQ.15:  2 point pentahedron element. 
EQ.16:  5 point 10-noded tetrahedron. 
EQ.17:  10-noded composite tetrahedron. 
EQ.18:  8 point enhanced strain solid element for linear statics only. 
EQ.19:  8-noded, 4 point cohesive element  
EQ.20:  8-noded,  4  point  cohesive  element  with  offsets  for  use  with 
shells  
EQ.21:  6-noded, 1 point pentahedron cohesive element  
EQ.22:  6-noded,  1  point  pentahedron  cohesive  element  with  offsets 
for use with shells  
EQ.23:  20-node solid formulation 
EQ.24:   27-node solid formulation 
EQ.41:  Mesh-free (EFG) solid formulation. 
EQ.42:  4-noded mesh-free (EFG) solid formulation. 
EQ.43:  Mesh-free enriched finite element. 
If  another  element  formulation  is  requested,  LS-DYNA  will  substitute,  when 
possible, one of the above in place of the one chosen.  The type 1 element, con-
stant stress, is generally much more accurate than the type 2 element, the selec-
tive reduced integrated element for implicit problems. 
3.  Element  for  Modified  Honeycomb  Material.    Element  formulations  0  and  9, 
applicable  only  to  *MAT_MODIFIED_HONEYCOMB,  behave  essentially  as
nonlinear  springs  so  as  to  permit  severe  distortions  sometimes  seen  in  honey-
comb  materials.    In  formulation  0,  the  local  coordinate  system  follows  the  ele-
ment rotation whereas in formulation 9, the local coordinate system is based on 
axes passing through the centroids of the element faces.  Formulation 0 is pre-
ferred  for  severe  shear  deformation  where  the  barrier  is  fixed  in  space.    If  the 
barrier  is  attached  to  a  moving  body,  which  can  rotate,  then  formulation  9  is 
usually preferred. 
4.  Elements  for  Shear  and  Pressure  Locking:  Types  2  and  18.    The  selective 
reduced  integrated  solid  element,  element  type  2,  assumes  that  pressure  is 
constant  throughout  the  element  to  avoid  pressure  locking  during  nearly  in-
compressible flow.  However, if the element aspect ratios are poor, shear lock-
ing will lead to an excessively stiff response.  A better choice, given poor aspect 
ratios, is the one point solid element which work well for implicit and explicit 
calculations.  For linear statics, the type 18 enhanced strain element works well 
with  poor  aspect  ratios.      Please  note  that  highly  distorted  elements  should 
always  be  avoided  since  excessive  stiffness  will  still  be  observed  even  in  the 
enhanced strain formulations. 
5.  Element  Type  99  for  Vibration.    Element  type  99  is  intended  for  vibration 
studies  carried  out  in  the  time  domain.    These  models  may  have  very  large 
numbers  of  elements  and  may  be  run  for  relatively  long  durations.    The  pur-
pose of this element is to achieve substantial CPU savings.  This is achieved by 
imposing strict limitations on the range of applicability, thereby simplifying the 
calculations: 
a)  Elements  must  be  cubed;  all  edges  must  parallel  to the global 𝑥-,  𝑦-  or 𝑧-
axis; 
b)  Small displacement, small strain, negligible rigid body rotation; 
c)  Elastic material only 
If these conditions are satisfied, the performance of the element is similar to the 
fully integrated S/R solid (ELFORM = 2) but at less CPU cost than the default 
solid  element  (ELFORM = 1).    Single  element  bending  and  torsion  modes  are 
included, so meshing guidelines are the same as for fully integrated solids – e.g.  
relatively  thin  structures  can  be  modeled  with  a  single  solid  element  through 
the thickness if required.  Typically, the CPU requirement per element-cycle is 
roughly two thirds that of the default solid element. 
No damping is included in the element formulation (e.g.  volumetric damping).  
It is strongly recommended that damping be applied, e.g.  *DAMPING_PART_-
MASS or *DAMPING_FREQUENCY_RANGE.
Δx84
Δx51
Δx62
Midsurface
Δx73
Figure 36-24.  Illustration of solid local coordinates. 
6.  8-Node Cohesive Element: Type 19.  Element type 19 is a cohesive element.  
The  tractions  on  the mid-surface  defined  as  the  mid-points  between  the  nodal 
pairs 1-5, 2-6, 3-7, and 4-8 are functions of the differences of the displacements 
between  nodal  pairs  interpolated  to  the  four  integration  points.    The  initial 
volume of the cohesive element may be zero, in which case, the density may be 
defined  in  terms  of  the  area  of  nodes  1-2-3-4.    See  Appendix  A  and  the  user 
material description for additional details.  See also *MAT_ADD_COHESIVE. 
The  tractions  are  calculated  in  the  local  coordinate  system  defined  at  the  cen-
troid of the element, see the Figure 36-24.  Defining the rotation matrix from the 
local to the global coordinate system at time 𝑡 as 𝐑(𝑡), the initial coordinates as 
𝐗,  and  the  current  coordinates  as  x,  the  displacements  at  an  integration  point 
are 
Δ𝐮 = 𝐑T(𝑡)Δ𝐱 − 𝐑T(0)Δ𝐗 
Δ𝐱 = ∑ 𝑁𝑖(𝑠, 𝑡)Δ𝐱𝑖+4,𝑖
𝑖=1
Δ𝐗 = ∑ 𝑁𝑖(𝑠, 𝑡)Δ𝐗𝑖+4,𝑖
𝑖=1
The  forces  are  obtained  by  integrating  the  tractions  over  the  mid-surface,  and 
rotating them into the global coordinate system.  It is the sum over integration 
points g = 1,2,3,4.
𝐅𝑖 = 𝐑(𝑡) ∑ 𝐓𝑔𝑁𝑖(𝑠𝑔, 𝑡𝑔) det(J𝑔)
,   for  1 ≤ 𝑖 ≤ 4,   and 𝐅𝑖+4 = −𝐅𝑖 
𝑔=1
Where, 
𝐓𝑔 = is the traction stress in the local coordinate system 
𝑁𝑖 = The shape function of the cohesive element at node i 
𝑠𝑔 and 𝑡𝑔 = The parameteric coordinates of the 4 integration points 
Jg = The  integration  point’s  portion  of  the  determinate  of  the  cohesive
element which is equivalent to the element volume 
7.  6-Node  Cohesive  Element:  Type  21.    Element  type  21  is  the  pentahedral 
counterpart to element type 19 with three nodes on the bottom and top surface.  
The  tractions  on  the  mid-surface  are  defined  as  the  mid-points  between  the 
nodal  pairs  1-5,  2-6,  and  3-7  are  functions  of  the  differences  of  the  displace-
ments between nodal pairs interpolated to one integration point.  The ordering 
of the nodal points in *ELEMENT_SOLID is given by:  
6-noded (cohesive) pentahedron  N1, N2, N3, N3, N5, N6, N7, N7, 0, 0  
Setting  ESORT.gt.0  in  *CONTROL_SOLID  will  automatically  sort  degenerated 
cohesive elements type 19 to cohesive pentahedron elements type 21. 
8.  Cohesive  Element  with  Offsets:  Types  20  and  22.    Element  type  20  is 
identical to element 19 but with offsets for use with shells.  The element is as-
sumed  to  be  centered  between  two  layers  of  shells  on  the  cohesive  element’s 
lower (1-2-3-4) and upper (5-6-7-8) surfaces.  The offset distances for both shells 
are one half the initial thicknesses of the nodal pairs (1-5, 2-6, 3-7, and 4-8) sepa-
rating the two shells.  These offsets are used with the nodal forces to calculate 
moments  that  are  applied  to  the  shells.    Element  type  20  in  tied  contacts  will 
work  correctly  with  the  option,  TIED_SHELL_EDGE_TO_SURFACE,  which 
transmits  moments.    Other  tied  options  will  leave  the  rotational  degrees-of-
freedom  unconstrained  with  the  possibility  that  the  rotational  kinetic  energy 
will cause a large growth in the energy ratio. 
Element  type  22  is  the  pentahedron  counterpart to  element  type  20  with  three 
nodes on the bottom and top surface.  The ordering of the nodal points in *ELE-
MENT_SOLID  are  identical  to  element  type  21  .    Setting  ES-
ORT.GT.0 in *CONTROL_SOLID will automatically sort degenerated cohesive 
elements type 20 to cohesive pentahedron elements type 22. 
9.  Automatic Sorting for EFG Background Mesh.  The current EFG formulation 
performs  automatic  sorting  for  finite  element  tetrahedral,  pentahedron,  and
hexahedral elements as the background mesh to identify the mesh-free geome-
try and provide the contact surface definition in the computation. 
10.  Essential  Boundary  Conditions.    The  mixed  transformation  method,  the 
coupled  FEM/EFG  method  and  the  fast  transformation  method  were  imple-
mented  in  EFG  3D  solid  formulation.   These  three  features  were  added  to  im-
prove the efficiency on the imposition of essential boundary conditions and the 
transfer  of  real  nodal  values  and  generalized  nodal  values.    The  mixed  trans-
formation  method  is  equivalent  to  the  full  transformation  method  with  im-
proved efficiency.  The behavior of the coupled FEM/EFG method is between 
FEM and EFG.  The fast transformation method provides the most efficient and 
robust results. 
11.  IDIM.  For compressible material like foam and soil, IDIM=1 is recommended.  
For  nearly  incompressible  material  like  metal  and  rubber,  IDIM=2  (default)  is 
recommended. 
12.  TOLDEF.    This  parameter  is  introduced  to  improve  the  negative  volume 
problem usually seen during large deformation analysis.  For the same analysis, 
the  larger  value  of  Toldef,  the  earlier  Semi-Lagrangian  or  Eulerian  kernel  is 
introduced  into  the  EFG  computation  and  more  cpu  time  is  expected.    Value 
between  0.0  and  0.1  is  suggested  in  the  crashworthiness  analysis.    Semi-
Lagrangian  kernel  is  suggested  for  the  solid  materials  and  Eulerian  kernel  is 
suggested for the fluid and E.O.S.  materials. 
13.  10-Node Tetrahedra: Types 16 and 17.  Formulations 16 and 17 are 10-noded, 
tetrahedral  formulations.    The  parameter  NIPTETS  in  *CONTROL_SOLID 
controls the number of integration points for these formulations.  Formulation 
17  is  generally  preferred  over  formulation  16  because,  unlike  16,  the  nodal 
weighting  factors  are  equal  and  thus  nodal  forces  from  contact  and  applied 
pressures are distributed correctly. 
When  applying  loads  to  10-noded  tetrahedrons  via  segments,  no  load  will  be 
applied to the midside nodes if the segments contain only corner nodes.  When 
defining  contact,  it  is  recommended  that  *CONTACT_AUTOMATIC_…  be 
used and the contact surface of the 10-noded tetrahedral part be specified by its 
part ID.  In this manner, midside nodes receive contact forces. 
If the 10-noded element connectivity is not defined in accordance with the fig-
ure  shown  in  *ELEMENT_SOLID,  the  order  of  the  nodes  can  be  quickly 
changed via a permutation vector specified with *CONTROL_SOLID.  If *ELE-
MENT_SOLID  defines  4-noded  tetrahedrons,  you  can  easily  convert  to  10-
noded  tetrahedrons  using  the  command  *ELEMENT_SOLID_TET4TOTET10.  
Because  the  characteristic  length  of  a  10-noded  tetrahedron  is  half  that  of  a  4-
noded tetrahedron, the time step for the tetrahedrons will be smaller by a factor 
of  2.    The  parameter  TET10  in  971,  when  set  to  1  in  *CONTROL_OUTPUT,
causes the full 10-node connectivity to be written to the d3plot and d3part data-
bases. 
14.  1-Point Nodal Pressure Tetrahedron: Type 13.  Element type 13 is identical 
with  type  10  but  with  additional  averaging  of  nodal  pressures,  which  signifi-
cantly  lowers  volumetric  locking.    Therefore,  it  is  well  suited  for  applications 
with  incompressible  and  nearly  incompressible  material  behavior,  i.e.    rubber 
materials or ductile metals with isochoric plastic deformations (e.g.  bulk form-
ing).  Compared to the standard tetrahedron (type 10), a speed penalty of max.  
25 % can be observed.  In implicit, all material models supported by type 10 are 
also  supported  for  this  element,  while  for  explicit  currently  material  models 
*MAT_001, 003, 006, 007, 015, 024, 027, 077, 081, 082, 091, 092, 098, 103, 106, 120, 
123, 124, 128, 129, 181, 183, 187, 224, 225, and 244  are fully supported.  For other 
materials this element behaves like the type 10 tetrahedron. 
15.  Fully Integrated S/R Solid Elements for Elements with Poor Aspect Ratio: 
Types  -1  and  -2.    Solid  formulations  -1  and  -2  may  offer  improved  behavior 
over formulation 2 by accounting for poor element aspect ratios in a manner so 
as to reduce the transverse shear locking effects seen in formulation 2.  Type -1 
is a more computationally efficient implementation of type -2, but a side-effect 
is that type -1’s resistance to a particular deformation mode, similar to an hour-
glass  mode,  is  weakened.    This  side  effect  is  not  truly  hourglassing  behavior 
and  so  there  is  no  hourglass  energy  and  behavior  is  not  affected  by  hourglass 
parameters. 
16.  EFG Solid Elements: Types 41 and 42.  EFG element type 41 supports 4-node, 
6-node and 8-node solid elements.  For 3D tetrahedron 𝑟-adaptive analysis (AD-
POPT=7  in  *CONTROL_ADAPTIVE  and  ADPOPT=2  in  *PART),  if  the  initial 
mesh is not purely comprised of tetrahedrons, element type 41 should be used 
instead  of  42  causing  the  mesh  to  be  converted  automatically  into tetrahedron 
after  the  first  time  step.    Element  type  42  only  supports  4-node  tetrahedron 
mesh, and is optimized to achieve better computational efficiency compared to 
41. 
17.  Smoothed Particle Galerkin (SPG) method: Type 47.  In SPG method, nodes 
are  converted  into  particles  and  4-node,  6-node  and  8-node  solid  elements  are 
supported.  The method is suitable for severe deformation problem and failure 
analysis.
*SECTION 
(Note:  NODE_SET option is available starting with the R3 release of Version 971) 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$$$$  *SECTION_SOLID 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$  A bolt modeled with solids was found to have excessive hourglassing. 
$  Thus, the section (sid = 116) associated with the bolt part was used 
$  to specify that a fully integrated Selectively-Reduced solid element 
$  formulation be used to totally eliminate the hourglassing (elform = 2). 
$ 
*SECTION_SOLID 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      sid    elform 
       116         2 
$ 
*PART 
bolts 
$      pid       sid       mid     eosid      hgid    adpopt 
        17       116         5 
$ 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
*SECTION_SPH_{OPTION} 
Available options include: 
<BLANK> 
ELLIPSE 
INTERACTION  
USER  
Purpose:  Define section properties for SPH particles. 
NOTE: This  feature  is  not  supported  for  use  in  implicit  cal-
culations. 
Card  Sets.    For  each  SPH  section  add  one  set  of  cards  1  or  2  (depending  on  the 
keyword option).  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SECID 
CSLH 
HMIN 
HMAX 
SPHINI 
DEATH 
START 
Type 
I/A 
F 
F 
F 
F 
F 
F 
Default 
none 
1.2 
0.2 
2.0 
0.0 
1.e20 
0.0 
Ellipse Card.  Additional card for ELLIPSE keyword option. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
HXCSLH  HYCSLH  HZCSLH 
HXINI 
HYINI 
HZINI 
Type 
F 
F 
F 
F 
F 
F 
  VARIABLE   
SECID 
DESCRIPTION
Section  ID.    SECID  is  referenced  on  the  *PART  card.    A  unique
number or label must be specified.
CSLH 
*SECTION 
DESCRIPTION
Constant  applied  to  the  smoothing  length  of  the  particles.    The
default  value  applies  for  most  problems.    Values  between  1.05
and 1.3 are acceptable.  Taking a value less than 1 is inadmissible.
Values larger than 1.3 will increase the computational time.  The 
default value is recommended. 
HMIN 
Scale factor for the minimum smoothing length  
HMAX 
Scale factor for the maximum smoothing length  
SPHINI 
Optional  initial  smoothing  length  (overrides  true  smoothing
length).    This  option  applies  to  avoid  LS-DYNA  to  calculate  the 
smoothing  length  during  initialization.    In  this  case,  the  variable
CSLH doesn't apply. 
DEATH 
Time imposed SPH approximation is stopped. 
START 
Time imposed SPH approximation is activated. 
Constant  applied  for  the  smoothing  length  in  the  𝑥-direction  for 
the ellipse case. 
Constant  applied  for  the  smoothing  length  in  the  𝑦-direction  for 
the ellipse case. 
Constant  applied  for  the  smoothing  length  in  the  𝑧-direction  for 
the ellipse case. 
Optional initial smoothing length in the 𝑥-direction for the ellipse 
case (overrides true smoothing length) 
Optional initial smoothing length in the 𝑦-direction for the ellipse 
case (overrides true smoothing length) 
Optional initial smoothing length in the 𝑧-direction for the ellipse 
case (overrides true smoothing length) 
HXCSLH 
HYCSLH 
HZCSLH 
HXINI 
HYINI 
HZINI 
Remarks: 
1.  Smoothing  Length.    The  SPH  processor  in  LS-DYNA  employs  a  variable 
smoothing  length.    LS-DYNA  computes  the  initial  smoothing  length,  ℎ0,  for 
each SPH part by taking the maximum of the minimum distance between every 
particle.    Every  particle  has  its  own  smoothing  length  which  varies  in  time 
according to the following equation:
𝑑𝑡
ℎ(𝑡) = ℎ(𝑡)∇ ⋅ v 
where  ℎ(𝑡)  is  the  smoothing  length,  and  where  ∇ ⋅ 𝐯  is  the  divergence  of  the 
flow.  The smoothing length increases as particles separate and reduces as the 
concentration increases.  This scheme is designed to hold constant the number 
of particles in each neighborhood.  In addition to being governed by the above 
evolution  equation  the  smoothing  length  is  constrained  to  be  between  a  user-
defined upper and lower value 
HMIN × ℎ0 < ℎ(𝑡) < HMAX × ℎ0. 
Defining  a  value  of  1  for  HMIN  and  1  for  HMAX  will  result  in  a  constant 
smoothing length in time and space. 
2.  USER  Option.    The  USER  option  allows  the  definition  of  customized  subrou-
tine  for  the variation of  the  smoothing  length.    A  subroutine  called hdot  is  de-
fined in the file dyn21.F (Unix/linux) or lsdyna.f (Windows). 
3.  Contact/Partial 
Interaction. 
  Combined  with  CONT=1 
the 
*CONTROL_SPH  card,  this  keyword  option  activates  a  partial  interaction  be-
tween SPH parts through the normal interpolation method and partially inter-
act through the contact option.  All the SPH parts defined using this keyword 
will interact with each other through normal interpolation method automatical-
ly.
in
*SECTION 
Purpose:  Define section properties for thick shell elements. 
Card Sets.  For each TSHELL section include a set of the following cards.  This input 
ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SECID 
ELFORM 
SHRF 
NIP 
PROPT 
QR 
ICOMP 
TSHEAR 
Type 
I/A 
Default 
none 
I 
1 
F 
1.0 
F 
2 
F 
1 
F 
0 
I 
0 
I 
0 
Angle  Cards.    If  ICOMP = 1  specify  NIP  angles  putting  8  on  each  card.    Include  as 
many cards as necessary. 
  Card 2 
Variable 
1 
B1 
Type 
F 
2 
B2 
F 
3 
B3 
F 
4 
B4 
F 
5 
B5 
F 
6 
B6 
F 
7 
B7 
F 
8 
B8 
F 
  VARIABLE   
SECID 
DESCRIPTION
Section  ID.    SECID  is  referenced  on  the  *PART  card.    A  unique
number or label must be specified. 
ELFORM 
Element formulation: 
EQ.1: one point reduced integration (default), 
EQ.2: selective reduced 2 × 2 in plane integration. 
EQ.3: assumed  strain  2 × 2  in  plane  integration,  see  remark 
below. 
EQ.5: assumed strain reduced integration with brick materials
EQ.6: assumed strain reduced integration with shell materials 
EQ.7:  assumed strain  2 × 2 in plane integration. 
SHRF 
Shear factor.  A value of 5/6 is recommended .
NIP 
*SECTION_TSHELL 
DESCRIPTION
Number  of  through  thickness  integration  points  for  the  thick
shell.  See the variable INTGRD in *CONTROL_SHELL for details 
of the through thickness integration rule. 
EQ.0: set to 2 integration points. 
PROPT 
Printout option: 
EQ.1.0: average resultants and fiber lengths, 
EQ.2.0: resultants at plan points and fiber lengths, 
EQ.3.0: resultants, stresses at all points, fiber lengths. 
QR 
Quadrature rule: 
LT.0.0:  absolute value is specified rule number, 
EQ.0.0: Gauss (up to five points are permitted), 
EQ.1.0: trapezoidal, not recommended for accuracy reasons. 
ICOMP 
Flag for layered composite material mode: 
EQ.1: a  material  angle  is  defined  for  each  through  thickness
integration point.  For each layer one integration point is
used. 
TSHEAR 
Flag for transverse shear strain or stress distribution : 
EQ.0.0: Parabolic, 
EQ.1.0: Constant through thickness. 
B1 
B2 
B3 
⋮ 
𝛽1, material angle at first integration point.  The same procedure
for  determining  material  directions  is  use  for  thick  shells  that  is
used for the 4 node quadrilateral shell. 
𝛽2, material angle at second integration point 
𝛽3, material angle at third integration point 
⋮  
BNIP 
𝛽NIP, material angle at eighth integration point
*SECTION 
1.  Thick  Shell  Element  Formulations.    Thick  shell  elements  are  bending 
elements that have 4 nodes on the bottom face and 4 on the top face.  Thick shell 
element  formulations  1,  2  and  6  are  extruded  thin  shell  elements  and  use  thin 
shell material models and have an uncoupled stiffness in the z-direction.  Thick 
shell  element  formulations  3,  5,  and  7  are  layered  brick  elements  that  use  3D 
brick  material  models.    Element  forms  3  and  5,  and  6  are  distortion  sensitive 
and should not be used in situations where the elements are badly shaped.  A 
single thick shell element through the thickness will capture bending response, 
but  with  element  types  3,  at  least  two  are  recommended  to  avoid  excessive 
softness. 
2.  Formulation  1  Quadrature  Quirk.    When  using  Gauss  quadrature  with 
element  formulation  1  the  number  of  integration  point  is  automatically 
switched to 3 when NIP = 2 and 5 when NIP = 4. 
3. 
Implicit  Time  Integration.    Thick  shell  elements  are  available  for  implicit 
analysis with the exception of thick shell formulation 1.  If an element of type 1 
is specified in an implicit analysis, it is internally switched to type 2 
4.  SHRF Field.  For ELFORM=1, 2 and 6, the transverse shear stiffness is scaled by 
the  SHRF  parameter.    Since  the  strain  is  assumed  to  be  constant  through  the 
thickness, setting SHRF=5/6 is recommended to obtain the correct shear ener-
gy.  For ELFORM=3 and 5, the SHRF parameter is not used, except for material 
types 33, 36, 133, 135, and 243.  For ELFORM=3, the shear stiffness is assumed 
constant  through the  thickness.      For  ELFORM=5,  6,  and  7, the  shear  distribu-
tion is assumed either parabolic if TSHEAR=0, or constant if TSHEAR=1.  The 
parabolic  assumption  is  good  when  the  elements  are  used  in  a  single  layer  to 
model  a  shell  type  structure,  but  the  constant  option  may  be  better  when  ele-
ments are stacked one on top of the other. 
5.  Modeling Composites.  Thick shell elements of all formulations can be used to 
model  layered  composites,  but  element  formulations  5  and  6  use  assumed 
strain  to  capture  the  complex  Poisson’s  effects  and  through  thickness  stress 
distribution  in  layered  composites.    To  define  the  layers  of  a  composite,  use 
QR < 0  to  point  to  *INTEGRATION_SHELL  data.    Alternatively,  the  *PART_-
COMPOSITE_TSHELL keyword offers a simplified way to define the layers. 
When modeling composites, laminated shell theory may be used to correct the 
transverse  shear  strain  if  the  shear  stiffness  varies  by  layer.    Laminated  shell 
theory is activated by setting LAMSHT = 4 or 5 on *CONTROL_SHELL.  When 
laminated  shell  theory  is  active,  the  TSHEAR  parameter  works  with  all 
ELFORM values to select either a parabolic or constant shear stress distribution.
The  keyword  *SENSOR  provides  a  convenient  way  of  activating  and  deactivating 
boundary conditions, airbags, discrete elements, joints, contact, rigid walls, single point 
constraints, and constrained nodes.  The sensor capability is new in the second release 
of  version  971  and  will  evolve  in  later  releases  to  encompass  many  more  LS-DYNA 
capabilities and replace some of the existing capabilities such as the airbag sensor logic.  
The keyword commands in this section are defined below in alphabetical order: 
*SENSOR_CONTROL 
*SENSOR_CPM_AIRBAG 
*SENSOR_DEFINE_CALC-MATH 
*SENSOR_DEFINE_ELEMENT 
*SENSOR_DEFINE_FORCE 
*SENSOR_DEFINE_FUNCTION 
*SENSOR_DEFINE_MISC 
*SENSOR_DEFINE_NODE 
*SENSOR_SWITCH 
*SENSOR_SWITCH_CALC-LOGIC 
*SENSOR_SWITCH_SHELL_TO_VENT 
To  define  and  utilize  a  sensor,  three  categories  of  sensor  keyword  commands  are 
needed as shown in Figure 37-1. 
1.  Sensors are defined using the *SENSOR_DEFINE commands.  Sensors provide 
a time history of model response that may be referred to by *SENSOR_SWITCH 
as  a  switching  criterion.    (Note:    The time  history  of  any  sensor  can  be  output 
using  the  SENSORD  function  in  *DEFINE_CURVE_FUNCTION  and  *DATA-
BASE_CURVOUT.) 
a)  *SENSOR_DEFINE(_ELEMENT,_FORCE,_MISC,_NODE) 
These commands define a sensor’s ID, type, and location.. 
b)  *SENSOR_DEFINE_CALC-MATH, *SENSOR_DEFINE_FUNCTION
*SENSOR_DEFINE
SENSORID TYPE
$ Perform math computation on sensor results
*SENSOR_DEFINE_CALC-MATH
SENSORID MATH SENSID1 SENSID2 ..
$Define switch criterion
*SENSOR_SWITCH
SWITCHID TYPE SENSORID LOGIC VAL
$Perform logic computation on SWITCH results
*SENSOR_SWITCH_CALC-LOGIC
SWITCHID SENSID1 SENSID2 ...
$Define how and what to switch
*SENSOR_CONTROL
CONTROL ID TYPE TYPE CNTC_ID
INIT_STA SWITCHID1 SWITCHID2
$Entity to be controlled by sensor
*CONTACT_......_ID
CNTC_ID
Figure 37-1.  Relationship between sensor keyword definitions. 
These commands define a sensor whose value is a mathmatical expression 
involving other sensors’ values. 
2.  Sensor  switching  criterion  definition  using  the  *SENSOR_SWITCH  keyword, 
which  can  be  combined  with  the  logical  calculation  command  *SENSOR_-
SWITCH_CALC-LOGIC  for  more  complicated  definitions.    The  logic  value 
yielded by this category of commands can be referred by *SENSOR_CONTROL 
to determine if a status switch condition is met. 
a)  *SENSOR_SWITCH 
This  command  compares  the  numerical  value  from  *SENSOR_DEFINE 
or *SENSOR_DEFINE_CALC-MATH with the given criterion to see if a 
switching condition is met. 
b)  *SENSOR_SWITCH_CALC-LOGIC 
This  command  performs  logical  calculation  on  the  information  from 
SENSOR_SWITCH. 
3.  Sensor  control  definition,  *SENSOR_CONTROL.    This  category  of  commands 
determines  how  and  what  to  switch  based  on  the  logical  values  from  *SEN-
SOR_SWITCH and/or *SENSOR_SWITCH_CALC-LOGIC.
*SENSOR 
Purpose:    This  command  uses  switches  (*SENSOR_SWITCH)  to  toggle  on  or  off  the 
effects of other LS-DYNA keywords such as *CONTACT, or *AIRBAG. 
Card Sets.  For each sensor control add a pair of cards 1 and 2.  This input ends at the 
next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CNTLID 
TYPE 
TYPEID 
TIMEOFF 
NREP 
Type 
I 
  Card 2 
1 
A 
2 
I 
3 
I 
4 
I 
5 
6 
7 
8 
Variable 
INITSTT 
SWIT1 
SWIT2 
SWIT3 
SWIT4 
SWIT5 
SWIT6 
SWIT7 
Type 
A 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
CNTLID 
Sensor control ID. 
TYPE 
Entity to be controlled: 
EQ.“AIRBAG”: 
*AIRBAG 
EQ.“BAGVENTPOP”:  Opening  and  closing  the  airbag  venting 
holes  
EQ.“BELTPRET”: 
Belt pretensioner firing  
EQ.“BELTRETRA”:  Locking the belt retractor 
EQ.“BELTSLIP”: 
Controling  the  slippage  of  slip  ring 
element  
EQ.“CONTACT”: 
*CONTACT 
EQ.“CONTACT2D”: 
*CONTACT_2D 
EQ.“CPM” 
*AIRBAG_PARTICLE 
EQ.“DEF2RIG”: 
*DEFORMABLE_TO_RIGID_AUTO-
MATIC
*SENSOR_CONTROL 
DESCRIPTION
EQ.“ELESET”:
Element set, see “ESTYP” below. 
EQ.“FUNCTION”: 
*DEFINE_CURVE_FUNCTION 
Remarks 5 & 6) 
(see 
EQ.“JOINT”: 
*CONSTRAINED_JOINT 
EQ.“JOINTSTIF”: 
*CONSTRAINED_JOINT_STIFFNESS 
EQ.“M PRESSURE”:  *LOAD_MOVING_PRESSURE 
EQ.“POREAIR”: 
*MAT_ADD_PORE_AIR 
EQ.“PRESC-MOT”: 
*BOUNDARY_PRESCRIBED_MOTION 
EQ.“PRESC-ORI”: 
*BOUNDARY_PRESCRIBED_ORIENTA-
TION_RIGID 
EQ.“PRESSURE”: 
*LOAD_SEGMENT_SET 
EQ.“RWALL”: 
*RIGID_WALL 
EQ.“SPC”: 
*BOUNDARY_SPC 
EQ.“SPOTWELD”: 
*CONSTRAINED_SPOTWELD 
TYPEID 
ID of entity to be controlled if TYPE is not set to FUNCTION.  If
TYPE is set to FUNCTION, see Remark 5.  For TYPE = POREAIR, 
TYPEID is the ID of the part containing material with pore air. 
TIMEOFF 
Flag for offset of time in curve:  
EQ.0: No offset is applied. 
EQ.1: Offset  the  abscissa  of  the  time-dependent  curve  by  the
time value at which the sensor is triggered. 
Type Of Control
Curve Affected 
PRESSURE 
PRESC-MOT 
PRESC-ORI 
*LOAD_SEGMENT 
*BOUNDARY_PRESCRIBED_MOTION 
*BOUNDARY_PRESCRIBED_ORIENTATION_RIGID 
Number of repeat of cycle of switches, SWITn, defined on the 2nd
card.  For example, a definition of SWITn like “601, 602, 601, 602, 
601,  602”  can  be  replaced  by  setting  NREP  to  3  and  SWITn  to 
”601,  602”.    Setting  NREP = -1  repeats  the  cycle  for  infinite 
number of times.  Default is 0. 
NREP
VARIABLE   
ESTYP 
DESCRIPTION
Type  of  element  set  to  be  controlled.    With  initial  status  set  to
“ON”,  all  the  elements  included  in  set  TYPEID  can  be  eroded
when the controller status is changed to “OFF”.  When TYPEID is
not defined, all elements of type ESTYP in the whole system will
be eroded. 
EQ.”BEAM”: 
Beam element set. 
EQ.”DISC”: 
Discrete element set 
EQ.”SHELL”: 
Thin shell element set  
EQ.”SOLID”: 
Solid element set 
EQ.”TSHELL”: 
Thick shell element set 
INITSTT 
Initial status: 
EQ.On:  Initial status is on 
EQ.Off:  Initial status is off 
ID  of  nth  switch.    At  the  start  of  the  calculation  SWIT1  is  active, 
meaning  that  it  controls  the  state  of  the  feature  specified  in
TYPEID.  After SWIT1 triggers, then SWIT2 becomes active; after
SWIT2  triggers,  then  SWIT3  becomes  active;  this  process  will
continue until the entire stack of switches has been exhausted. 
SWITn 
Remarks: 
1.  Activation  of  Bag  Venting.    BAGVENTPOP  activates  (opens)  or  deactivates 
(closes)  the  venting  holes  of  *AIRBAG_HYBRID  and  *AIRBAG_WANG_
NEFSKE.    It  overwrites  the  definitions  of  PVENT  of  *AIRBAG_HYBRID  and 
PPOP  of  *AIRBAG_WANG_NEFSKE.    More  than  one  SWIT  can  be  input  to 
open/close initially closed/opened holes, and then reclose/reopen the holes. 
2.  Seatbelt  Retractors.    The  locking  (or  firing)  of  seatbelt  retractor  (or  preten-
sioner) can be controlled through either general sensor, option BELTRETRA (or 
BELTPRET), or seatbelt sensors, *ELEMENT_SEATBELT_SENSOR.  When BEL-
TRETRA  (or  BELTPRET)  is  used,  the  SBSIDi  in  *ELEMENT_SEATBELT_RE-
TRACTOR (or PRETENSIONER) should be left blank. 
3.  Seatbelt Slip Ring.  For one-way slip ring, a non-zero DIRECT in *ELEMENT_-
SEATBELT_SLIPRING, BELTSLIP activates the constraint of one-way slippage 
when the status of SENSOR_CONTROL is on.  When the SENSOR_CONTROL 
is turned off, the one-way slippage constraint is deactivated, therefore allowing 
slippage in both directions.
To  model  a  two-way  slip  ring,  BELTSLIP  allow  slippage  in  both  directions 
when the status of SENSOR_CONTROL is on.  When the status of SENSOR_-
CONTROL is off, the slip ring lockup happens, no slippage is allowed then. 
4.  Switching  Between  Rigid  and  Deformable.    DEF2RIG  provides  users  more 
flexibility controlling material switch between rigid and deformable.  Status of 
ON trigger the switch and deformable material becomes rigid.  Rigidized mate-
rial can then return to deformable status when status becomes OFF.  As many 
as  7  SWITs  can  be  input,  any  of  them  will  change  the  status  triggered  by  its 
preceding SWIT or the initial condition, INTSTT. 
5.  Function for Sensor Control.  When the input parameter TYPE of *SENSOR_-
CONTROL is set to "FUNCTION", the function "SENSOR(cntlid)" as described 
in *DEFINE_CURVE_FUNCTION takes on a value that depends on the current 
status of the *SENSOR_CONTROL.  That status is either on or off at any given 
point in time.  If the status is on, the value of function SENSOR(cntlid) is simply 
set  to  the  integer  value  1.    If  the  status  is  off,  the  value  of  function  SEN-
SOR(cntlid)  is  set  to  the  input  parameter  TYPEID  (an  integer)  as  specified  in 
*SENSOR_CONTROL.    To  help  clarify  this  relationship  between  *SENSOR_-
CONTROL  and  *DEFINE_CURVE_FUNCTION,  consider  the  following  exam-
ple. 
6.  Example  of  Function  Sensor  Control.    Suppose  a  *SENSOR_CONTROL 
defined with CNTLID=101, TYPE="FUNCTION", and TYPEID = -2 has a status 
of  off.    Then  a  *DEFINE_CURVE_FUNCTION  defined  as  “2+3*sensor(101)” 
will have a value of 2 + 3(-2) = -4.  On the other hand, if the status of the *SEN-
SOR_CONTROL  changes  to  on, the  *DEFINE_CURVE_FUNCTION  takes on a 
value of 2 + 3(1) = 5.
*SENSOR 
Purpose:    This  command  will  associate  a  CPM  airbag  with  a  sensor  switch  .    When  the  condition  flag  is  raised,  the  specified  CPM  airbag  will 
deploy.    All  time  dependent  curves  used  for  the  CPM  airbag  are  shifted  by  the 
activation  time  including  the  *AIRBAG_PARTICLE  curves  for  the  inflator  and  vent  as 
well as the *MAT_FABRIC curves for TSRFAC. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CPMID 
SWITID 
TBIRTH 
TDEATH 
TDR 
DEFPS 
RBPID 
Type 
I 
I 
F 
F 
F 
I 
I 
  VARIABLE   
DESCRIPTION
CPMID 
Bag ID of *AIRBAG_PARTICLE_ID 
SWITID 
Switch ID of *SENSOR_SWITCH 
TBIRTH 
If SWITID is set, TBIRTH is not active.  If SWITID is 0, TBIRTH is
the activation time for the bag with ID = CPMID.  All of the time 
dependent  curves  that  are  used  in  this  bag  will  be  offset  by  the 
value of TBIRTH. 
TDEATH 
Disable  the  CPMID  bag  when  the  simulation  time  exceeds  this
value. 
TDR 
DEFPS 
If  TDR  is  greater  than  0  the  bag  with  ID =  CPMID  will  be  rigid 
starting at first cycle and switch to deformable at time TDR. 
Part  set  ID  specifiying  which  parts  of  the  bag  with  ID =  CPMID 
are deformable. 
RBPID 
Part ID of the master rigid body to which the part is merged.
*SENSOR_DEFINE_CALC-MATH 
Purpose:    Defines  a  new  sensor  with  a  unique  ID.    The  values  associated  with  this 
sensor  are  computed  by  performing  mathematical  calculations  with  the  information 
obtained from sensors defined by the *SENSOR_DEFINE_OPTION. 
Math  Sensor  Cards.    Include  one  additional  card  for  each  math  sensor.    This  input 
ends at the next keyword (“*”) card. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SENSID 
CALC 
SENS1 
SENS2 
SENS3 
SENS4 
SENS5 
SENS6 
Type 
I 
A 
I 
I 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
SENSID 
Sensor ID. 
Mathematical calculation, See Table 37-2. 
ith Sensor ID 
CALC 
SENSi 
Remarks: 
All sensors, SENSi, defined with either SENSOR_DEFINE_NODE_SET or SENSOR_DE-
FINE_ELEMENT_SET, must refer to either the same node set or the same element set. 
Example: 
$ 
$ assume set_2 to have 100 solid elements 
*SENSOR_DEFINE_ELEMENT_SET 
$ this sensor traces xx-strain of all 100 solid elements in set-2 
        91     SOLID        -2        XX    STRAIN 
*SENSOR_DEFINE_ELEMENT_SET 
$ this sensor traces yy-strain of all 100 solid elements in set-2 
        92     SOLID        -2        YY    STRAIN 
*SENSOR_DEFINE_ELEMENT_SET 
$ this sensor traces zz-strain of all 100 solid elements in set-2 
        93     SOLID        -2        ZZ    STRAIN 
*SENSOR_DEFINE_CALC-MATH 
$ this sensor traces strain magnitudes of all 100 solid elements in set-2 
       104  SQRTSQRE        91        92        93         0         0         0 
*SENSOR_SWITCH 
$ Because ELEMID of *sensor_define_element_set was input as "-2", SWITCH-1 will be  
$ turned on if at least one of 100 elements has a strain magnitude>2.0E-4 
$ On the other hand, If ELEMID was input as "2", SWITCH-1 will be turned on if 
$ all 100 elements have strain magnitudes>2.0E-4 
         1    SENSOR       104        GT    2.0E-4         0     0.001 
$
ABSSUM 
MIN 
MAX 
MAXMAG 
MINMAG 
MULTIPLY 
*SENSOR_DEFINE_CALC-MATH 
*SENSOR 
FUNCTION 
DESCRIPTION 
Absolute value of the sum of sensor 
values 
MATHEMTAICAL FORM 
|SENS1 + SENS2 + ⋯ |
The minimum of sensor values 
min(SENS1,SENS2, … )
The maximum of sensor values 
max(SENS1,SENS2, … )
The maximum of magnitude of sensor 
values 
The minimum of the magnitude of 
sensor values 
Multiplication of sensor values; 
negative for division (performed left to 
right) 
max(|SENS1|, |SENS2|, … )
min(|SENS1|, |SENS2|, … )
SENS1 × SENS2 × ⋯
SQRE 
Summation of squared values of 
sensor values 
SQRTSQRE 
Square root of the sum of squared 
values 
SENS12 + SENS22 + ⋯ 
√SENS12 + SENS22 + ⋯ 
SQRT 
Summation of square root of sensor 
values; negative for subtracting values 
√SENS1 + √SENS2
+ ⋯
SUMABS 
Summation of absolute sensor values 
|SENS1| + |SENS2| + ⋯
SUM 
Summation of sensor values; negative 
for subtracting values 
SENS1 + SENS2 + ⋯
Table 37-2.  Available mathematical functions.
*SENSOR_DEFINE_ELEMENT_{OPTION} 
Available options include: 
<BLANK> 
SET 
Purpose:    Define  a  strain  gage  type  element  sensor  that  checks  the  stress,  strain,  or 
resultant force of an element or element set. 
Element  Sensor  Cards.    Include  one  additional  card  for  each  element  sensor.    This 
input ends at the next keyword (“*”) card. 
Card 
1 
2 
3 
4 
5 
6 
Variable 
SENSID 
ETYPE 
ELEMID 
COMP 
CTYPE 
LAYER 
Type 
I 
A 
I 
A 
A 
A/I 
7 
SF 
R 
8 
PWR 
R 
Optional card for SET option.   
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SETOPT 
Type 
A 
  VARIABLE   
DESCRIPTION
SENSID 
Sensor ID. 
ETYPE 
Element type.  Available options include: 
EQ.BEAM: 
beam element. 
EQ.SHELL: 
shell element 
EQ.SOLID: 
solid element 
EQ.DISC-ELE:  discrete element 
EQ.SEATBELT: seatbelt element 
EQ.TSHELL: 
thick shell element
VARIABLE   
ELEMID 
DESCRIPTION
Element ID or element set ID when option_SET is active.  In case 
of option_SET, a positive ELEMID requires all elements in set EL-
EMID to meet the switch condition to switch the status of related
*SENSOR_SWITCH.  If ELEMID is negative, the status of related 
*SENSOR_SWITCH will be changed if at least one of elements in
set “-ELEMID” meets the switch condition. 
COMP 
Component  type.    The  definition  of  component,  and  its  related
coordinate  system,  is  consistent  with  that  of  elout.    Leave  blank 
for  discrete  elements.    Available  options  for  elements  other  than
discrete element include: 
EQ.XX: 
EQ.YY: 
EQ.ZZ: 
EQ.XY: 
EQ.YZ: 
EQ.ZX: 
𝑥-normal component for shells and solids 
𝑦-normal component for shells and solids 
𝑧-normal component for shells and solids 
𝑥𝑦-shear component for shells and solids 
𝑦𝑧-shear component for shells and solids 
𝑧𝑥-shear component for shells and solids 
EQ.AXIAL: 
axial 
EQ.SHEARS: local 𝑠-direction 
EQ.SHEART:  local 𝑡-direction 
CTYPE 
Sensor type.  Available options include: 
EQ.STRAIN: 
strain component for shells and solids 
EQ.STRESS:  stress component for shells and solids 
EQ.FORCE: 
resultants 
seatbelt,  or 
force 
translational discrete element; moment resultant
for rotational discrete element 
for  beams, 
EQ.MOMENT:  moment resultants for beams 
EQ.DLEN: 
change in length for discrete or seatbelt element
EQ.FAIL: 
failure  of  element,  sensor  value  =  1  when 
element fails, = 0 otherwise.
LAYER 
*SENSOR_DEFINE_ELEMENT 
DESCRIPTION
Layer of integration point in shell or thick shell element.  Options
include: 
EQ.BOT: component  at  lower  surface  meaning  the  integration
point  with  the  smallest  through-the-thickness  local 
coordinate 
EQ.TOP:  component  at  upper  surface  meaning  the  integration 
point  with  the  largest through-the-thickness  local  co-
ordinate 
When  CTYPE = STRESS,  LAYER  could  be  an  integer  “I”  to
monitor the stress of the I’the integration point. 
SF, PWR 
Optional  parameters,  scale  factor  and  power,  for  users  to  adjust 
the resultant sensor value.  The resultant sensor value is 
[SF × (Original Value)]PWR
SETOPT 
Option to process set of data when SET option is specified.  More
details  can  be  found  in  *SENSOR_DEFINE_NODE_SET.    When 
SETOPT  is  defined,  a  single  value  will  be  reported,  which  could
be 
EQ.AVG:  the average value of the dataset 
EQ.MAX:  the maximum value of the dataset 
EQ.MIN:  the minimum value of the dataset 
EQ.SUM:  the sum of the dataset
Purpose:  Define a force transducer type sensor. 
*SENSOR 
Force  Sensor  Cards.    Include  one  additional  card  for  each  force  sensor.    This  input 
ends at the next keyword (“*”) card. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SENSID 
FTYPE 
TYPEID 
VID 
CRD 
Type 
I 
A 
I 
A/I 
I 
  VARIABLE   
DESCRIPTION
SENSID 
Sensor ID. 
FTYPE 
Force type.  See Table 37-3. 
TYPEID 
ID  defined  in  the  associated  KEYWORD  command.    See  Table 
37-3. 
VID 
Vector along which the forces is measured. 
EQ.X: 
EQ.Y: 
EQ.Z: 
𝑥-direction in coordinate system CRD. 
𝑦-direction in coordinate system CRD. 
𝑧-direction in coordinate system CRD. 
EQ.XMOMENT:  𝑥-direction  moment  for  JOINT,  JOINTSTIF, 
PRESC-MOT or SPC. 
EQ.YMOMENT: 𝑦-direction  moment  for  JOINT,  JOINTSTIF, 
PRESC-MOT or SPC. 
EQ.ZMOMENT:  𝑧-direction  moment  for  JOINT,  JOINTSTIF, 
PRESC-MOT or SPC. 
VID∈{INT}: 
vector ID n in coordinate system CRD. 
CRD 
Optional  coordinate  system,  defined  by  *DEFINE_COORDI-
NATE_NODES,  to  which  vector  VID  is  attached.    If  blank  the
global coordinate system is assumed.
FTYPE 
TYPEID 
(Enter ID defined in following 
KEYWORD commands) 
OUTPUT 
ASCII 
FILE 
AIRBAG 
*AIRBAG 
Airbag pressure 
ABSTAT 
CONTACT 
*CONTACT 
CONTACT2D 
*CONTACT_2D 
CPM 
*AIRBAG_PARTICLE 
JOINT 
*CONSTRAINED_JOINT 
JOINTSTIF 
*CONSTRAINED_JOINT_STIFFNESS 
PRESC-MOT 
*BOUNDARY_PRESCRIBED_MOTION 
RWALL 
*RIGIDWALL 
SPC 
*BOUNDARY_SPC 
Contact force on 
the slave side 
Contact force on 
the slave side 
Airbag pressure 
Joint force 
Joint stiffness 
force 
Prescribed 
motion force 
RCFORC 
RCFORC 
AB-
STAT_CPM
JNTFORC 
JNTFORC 
BNDOUT 
Rigid wall force 
RWFORC 
SPC reaction 
force 
SPCFORC 
SPOTWELD 
*CONSTRAINED_POINTS 
Spot weld force 
SWFORC 
X-SECTION 
*DATABASE_CROSS_SECTION 
Section force 
SECFORC 
Table 37-3. Force transducer type sensor
*SENSOR 
Purpose:  Defines a new sensor with a unique ID.  The value associated with this sensor 
is  computed  by  performing  mathematical  calculations  defined  in  *DEFINE_FUNC-
TION, with the information obtained from other sensors defined by the *SENSOR_DE-
FINE_OPTION. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SENSID 
FUNC 
SENS1 
SENS2 
SENS3 
SENS4 
SENS5 
SENS6 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Sensor Cards.  Additional Cards needed when SENS1 < -5.  Include as many cards as 
needed to specify all |SENS1| cards. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SENSi 
SENSi+1  SENSi+2  SENSi+3 SENSi+4 SENSi+5  SENSi+6  SENSi+7 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
SENSID 
Sensor ID 
FUNC 
SENS1 
Function ID 
1st Sensor ID, the value of which will be used as the 1st argument
of  function  FUNC.    If  defined  as  negative,  the  absolute  value  of
SENS1,  |SENS1|,  is  the  number  of  sensors  to  be  input.    If
|SENS1| > 5,  additional  cards  will  be  needed  to  input  the  ID  of
all sensors.  The number of sensor is limited to 15. 
SENSi 
ith Sensor ID, the value of which will be used as the ith argument 
of function FUNC
*SENSOR_DEFINE_MISC 
Purpose:    Trace  the  value  of  a  miscellaneous  item.    This  card  replaces  *SENSOR_DE-
FINE_ANGLE. 
Force Sensor Cards.  Include one additional card for each miscellaneous sensor.  This 
input ends at the next keyword (“*”) card. 
Card 
1 
2 
3 
Variable 
SENSID  MTYPE 
4 
I1 
5 
I2 
6 
I3 
7 
I4 
8 
I5 
Type 
I 
A 
I/A 
I/A 
I/A 
I/A 
I/A 
  VARIABLE   
DESCRIPTION
SENSID 
Sensor ID.
VARIABLE   
DESCRIPTION
MTYPE 
Entity to be traced: 
EQ.ANGLE: 
Angular  accelerometer  sensor  tracing  the 
angle  between  two  lines,  0≤  θ  ≤180.    The 
fields  I1  and  I2  are  node  numbers  defining 
the  1st  line,  while  I3  and  I4  are  node  num-
bers defining the 2nd line. 
EQ.CURVE:       The  value of a time-dependent curve defined 
or 
by 
*DEFINE_CURVE_FUNCTION 
*DEFINE_CURVE.  I1 is the curve ID. 
EQ.RETRACTOR: The  seatbelt  retractor  payout  rate  is  traced. 
I1 is the retractor ID. 
EQ.RIGIDBODY:  Accelerometer  sensor  tracing  the  kinematics 
of a rigid body with id I1.  The I2 field speci-
fies  which  kinematical  component  is  to  be 
traced.  It may be set to “TX”, “TY”, or “TZ” 
for  𝑋,  𝑌,  and  𝑍  translations  and  to  “RX”, 
“RY”,  or  “RZ”  for  the  𝑋,  𝑌,  and  𝑍  compo-
nents  of  the  rotation.    The  I3  field  specifies 
the  kinematics  type:  “D”  for  displacement, 
“V”  for  velocity  and  “A”  for  acceleration. 
Output  is  calculated  with  respect  to  the 
global coordinate system when the I4 field is 
set  to  “0”,  its  default  value;  the  local  rigid-
body  coordinate  system  is  used  when  I4  is 
set to “1”. 
EQ.TIME: 
The current analysis time is traced.   
I1, …, I5 
See MTYPE.
*SENSOR_DEFINE_NODE_{OPTION} 
Available options include: 
<BLANK> 
SET 
Purpose:    Define  an  accelerometer  type  sensor.    This  command  outputs  the  relative 
linear  acceleration,  velocity,  or  relative  coordinate  of  node-1  with  respect  to  node-2 
along vector VID. 
Node  Sensor  Cards.    Include  one  additional  card  for  each  node  sensor.    This  input 
ends at the next keyword (“*”) card. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SENSID 
NODE1 
NODE2 
VID 
CTYPE 
SETOPT 
Type 
I 
I 
I 
I 
A 
A 
  VARIABLE   
DESCRIPTION
SENSID 
Sensor ID. 
NODE1,2 
Nodes defining the accelerometer.  NODE1 is a node set ID when
option_SET is active.  In case of option_SET, and when SETOPT is 
not defined, a positive NODE1 requires all nodes in set NODE1 to
meet  the  switch  condition  to  switch  the  status  of  related  *SEN-
SOR_SWITCH.  If NODE1 is negative, the status of related *SEN-
SOR_SWITCH  will  be  changed  if  at  least  one  of  nodes  in  set  “-
NODE1” meets the switch condition. 
VID 
ID of vector along which the nodal values are measured, see *DE-
FINE_VECTOR.    The  magnitude  of  nodal  values  (coordinate,
velocity or acceleration) will be output if VID is 0 or undefined. 
CTYPE 
Output component type (character string). 
EQ.ACC: 
acceleration 
EQ.VEL: 
velocity 
EQ.COORD: coordinate 
EQ.TEMP: 
temperature
VARIABLE   
SETOPT 
DESCRIPTION
Option to process set of data when SET option is specified.  When
SETOPT is specified, a single value will be reported, which could
be 
EQ.AVG:  the average value of the dataset 
EQ.MAX:  the maximum value of the dataset 
EQ.MIN:  the minimum value of the dataset 
EQ.SUM:  the sum of the dataset 
Remarks: 
1.  Time  Evolution  of  Vector  VID.    The  vector  direction  is  determined  by  *DE-
FINE_VECTOR.  This vector direction is updated with time only if the coordi-
nate system CID  is defined using *DEFINE_COORDI-
NATE_NODES  and  the  parameter  FLAG  is  set  to  1.    Otherwise,  the  vector 
direction is fixed. 
2.  SETOPT.  When SETOPT is not defined for SET option, a list of nodal data will 
be reported, one for each node in the node set.  These reported nodal values can 
be  processed  by  *SENSOR_DEFINE_FUNCTION  and  *SENSOR_DEFINE_-
CALC-MATH, and then result in a list of processed values.  These nodal values 
can  be  used  to  determine  if  the  status  of  SENSOR_SWITCH  will  be  changed.  
Depending on the sign of NODE1, it can take only one single data point or the 
whole data sets to meet the switch condition to change the status of the related 
SENSOR_SWITCH.  It should be note that all sensor definitions referred to by 
these  two  processing  commands  must  have  the  same  number  of  data  points.  
The  reported  nodal  values  cannot  be  accessed  by  commands  like  *DEFINE_-
CURVE_FUNCTION, see SENSORD option.   
When SETOPT is defined, the nodal values of all nodes in the node set will be 
processed,  depending  on  the  definition  of  SETOPT,  the  resulting  value  is  re-
ported as the single sensor value.  The reported value can be processed by both 
*SENSOR_DEFINE_FUNCTION and *SENSOR_DEFINE_CALC-MATH as well 
as  other  regular  sensors.    This  reported  value  can  also  be  accessed  by  *  DE-
FINE_CURVE_FUNCTION  using  SENSORD  option.    If  the  reference  node, 
node2, is needed, NODE2 has to be a node set containing the same number of 
nodes as node set “-NODE1”.  The nodes in sets “-NODE1” and “NODE2” have 
to be arranged in the same sequence so that the nodal value of nodes in set “-
NODE1” can be measured with respect to the correct node in set NODE2. 
3.  When NODE1 is a node that belongs to a rigid body and CTTYPE=”ACC”, the 
acceleration  recorded  by  the  sensor  is  not  updated  every  time  step  but  rather
only  when  nodal  output  is  written  according  to  *DATABASE  commands.    As 
an  alternative,    *SENSOR_DEFINE_MISC  with  MTYPE=”RIGIDBODY”  up-
dates the sensor data every time step.
*SENSOR 
Purpose:    This  command  compares  the  value  of  a  sensor,  *SENSOR_DEFINE  or  SEN-
SOR_CALC-MATH,  to  a  given  criterion  to  check  if  the  switch  condition  is  met.    It 
output a logic value of TRUE or FALSE. 
Sensor Switch Cards.  Include one additional card for each sensor switch.  This input 
ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SWITID 
SENSID 
LOGIC 
VALUE 
FILTRID 
TIMWIN 
Type 
I 
I 
A 
F 
I 
F 
  VARIABLE   
SWITID 
DESCRIPTION
Switch  ID  can  be  referred  directly  by  *SENSOR_CONTROL  to 
control the status of entities like CONTACT and AIRBAG, or can 
be  referred  to  by  *SENSOR_SWITCH_CALC-LOGIC  for  logic 
computation. 
SENSID 
ID of the sensor whose value will be compared to the criterion to
determine if a switch condition is met. 
LOGIC 
Logic operator, could be either LT (<) or GT (>). 
VALUE 
Critical value 
FILTER 
TIMWIN 
Filter  ID  (optional).    Filters  may  be  defined  using  *DEFINE_FIL-
TER. 
Trigger a status change when the value given by the sensor is less
than  or  greater  than  (depending  on  LOGIC)  the  VALUE  for  a
duration defined by TIMWIN.
*SENSOR_SWITCH_CALC-LOGIC 
Purpose:  This command performs a logic calculation for the logic output of up to seven 
*SENSOR_SWITCH or *SENSOR_SWITCH_CALC-LOGIC definitions.  The output is a 
logic value of either TRUE or FALSE. 
Log Cards.  Include one additional card for each logic rule.  This input ends at the next 
keyword (“*”) card. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SWITID 
SWIT1 
SWIT2 
SWIT3 
SWIT4 
SWIT5 
SWIT6 
SWIT7 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
SWITID 
DESCRIPTION
Switch  ID  can  be  referred  directly  by  *SENSOR_CONTROL  to 
control the status of entities like CONTACT and AIRBAG, or can 
be  referred  to  by  *SENSOR_SWITCH_CALC-LOGIC  for  logic 
computation. 
SWITn 
Input a positive sensor switch ID for "AND" and negative sensor
switch ID for "OR".  SWIT1 must always be positive. 
This keyword implements standard Boolean logic. 
true = 1, 
false = 0, 
and = multiplication, 
or = addition 
An expression evaluating to 0 is false, while any expression that evaluates to greater than 0 is 
true, and, therefore, set to 1. 
Example: 
Consider 5 switches defined as follows: 
switch(11) = true 
switch(12) = false 
switch(13) = true 
switch(14) = true
To evaluate the expression 
switch(15) = false. 
[switch(11) or switch(12) or switch(13)] and [switch(14) or switch(15)] 
and assign the value to switch(103), the following would apply: 
*SENSOR_SWITCH_CALC-LOGIC
101,11,-12,-13 
102,14,-15 
103,101,102 
This translates into 
switch(101) = switch(11) or switch(12) or switch(13) 
= min((1  +  0  +  1), 1) 
= 1 (true)  
switch(102) = switch(14) or switch(15)  
= min((1 + 0), 1)  
= 1 (true) 
switch(103) = switch(101) and switch(102) 
= min((1 × 1), 1) 
= 1 (true) 
Therefore, 
switch(101)=true
⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞
[switch(11) or 𝑠witch(12) or switch(13)] 
switch(102)=true
⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞
AND  [switch(14) or switch(15)]
= switch(103)
= true
*SENSOR_SWITCH_SHELL_TO_VENT 
Purpose:    This  option  will  treat  the  failed  shell  elements  as  vent  hole  for  the  airbag 
defined by *AIRBAG_PARTICLE.  The mass escaped from the vent will be reported in 
abstat_cpm file. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
ITYPE 
C23 
Type 
I 
I 
F 
Shell  Fail  Time  Cards.    Optional  Cards  for  setting  time  at  which  shells  in  a  shell  list 
  change  into  vents.    This  card  may  be  repeated  up  time  15  times. 
This input ends at the next keyword (“*”) cards. 
 Optional 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
FTIME 
C23V 
Type 
I 
F 
F 
Default 
none 
0. 
C23 
  VARIABLE   
DESCRIPTION
ID 
TYPE 
Part set ID/Part ID. 
EQ.0: Part 
EQ.1: Part set 
C23 
Vent Coefficient (Default = 0.7) 
LT.0: User  defined  load  curve  ID.    The vent  coefficient  will  be
determined by this pressure-vent_coeff curve. 
SSID 
ID of *SET_SHELL_LIST 
FTIME 
Time to convert shell list to vent.  (Default is from t = 0.)
VARIABLE   
DESCRIPTION
C23V 
Vent Coefficient (Default = C23) 
LT.0: User  defined  load  curve  ID.   The vent  coefficient  will  be
determined by this pressure-vent_coeff curve.
The  keyword  *SET  provides  a  convenient  way  of  defining  groups  of  nodes,  parts, 
elements,  and  segments.    The  sets  can  be  used  in  the  definitions  of  contact  interfaces, 
loading conditions, boundary conditions, and other inputs.  The keyword provides also 
a  convenient  way  of  defining  groups  of  vibration  modes  to  be  used  in  frequency 
domain  analysis.    Each  set  type  must  have  a  unique  numeric  identification.    The 
keyword control cards in this section are defined in alphabetical order: 
*SET_BEAM_{OPTION}_{OPTION} 
*SET_BEAM_ADD 
*SET_BEAM_INTERSECT 
*SET_BOX 
*SET_DISCRETE_{OPTION}_{OPTION} 
*SET_DISCRETE_ADD 
*SET_MODE_{OPTION} 
*SET_MULTIMATERIAL_GROUP_LIST 
*SET_NODE_{OPTION}_{OPTION} 
*SET_NODE_ADD_{OPTION} 
*SET_NODE_INTERSECT 
*SET_PART_{OPTION}_{OPTION} 
*SET_PART_ADD 
*SET_SEGMENT_{OPTION}_{OPTION} 
*SET_SEGMENT_ADD 
*SET_SEGMENT_INTERSECT 
*SET_2D_SEGMENT_{OPTION}_{OPTION} 
*SET_SHELL_{OPTION}_{OPTION} 
*SET_SHELL_ADD 
*SET_SHELL_INTERSECT
*SET_SOLID_ADD 
*SET_SOLIDT_INTERSECT 
*SET_TSHELL_{OPTION}_{OPTION} 
An additional option_TITLE may be appended to all the *SET keywords.  If this option 
is used then an addition line is read for each section in 80a format which can be used to 
describe  the  set.    At  present  LS-DYNA  does  make  use  of  the  title.    Inclusion  of  titles 
gives greater clarity to input decks. 
The GENERAL option is available for set definitions.  In this option, the commands are 
executed in the order defined.  For example, the delete option cannot delete a node or 
element unless the node or element was previously added via a command such as BOX 
or ALL. 
The COLLECT option allows for the definition of multiple sets that share the same ID 
and  combines  them  into  one  large  set  whenever  this  option  is  found.    If  two  or  more 
like sets definitions share the same IDs, they are combined if and only if the_COLLECT 
option is specified in each definition.  If the_COLLECT option is not specified for one or 
more  like  set  definitions  that  share  identical  ID’s  an  error  termination  will  occur.    For 
include  files  using  *INCLUDE_TRANSFORM  where  set  offsets  are  specified,  the 
offsets are not applied for the case where the_COLLECT option is present.
*SET_BEAM_{OPTION1}_{OPTION2} 
For OPTION1 the available options are: 
<BLANK> 
GENERATE 
GENERATE_INCREMENT 
GENERAL 
For OPTION2 the available option is: 
COLLECT 
The GENERATE and GENERATE_INCREMENT options will generate block(s) of beam 
element  ID’s  between  a  starting ID  and  an  ending  ID.    An  arbitrary  number  of  blocks 
can be specified to define the set. 
Purpose:    Define  a  set  of  beam  elements  or  a  set  of  seat  belt  elements  . 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
Type 
I 
Default 
none 
Beam  Element  ID  Cards.    This  Card  2  format  applies  to  the  case  of  an  unset 
(<BLANK>)  keyword  option.    Set  one  value  per  element  in  the  set.    Include  as  many 
cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 2 
Variable 
1 
K1 
Type 
I 
2 
K2 
I 
3 
K3 
I 
4 
K4 
I 
5 
K5 
I 
6 
K6 
I 
7 
K7 
I 
8 
K8
Beam Element Range Cards.  This Card 2 format applies to the GENERATE keyword 
option.  Set one pair of BNBEG and BNEND values per block of elements.  Include as 
many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
B1BEG 
B1END 
B2BEG 
B2END 
B3BEG 
B3END 
B4BEG 
B4END 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Beam Element Range with Increment Cards.  This Card 2 format applies to the GEN-
ERATE_INCREMENT keyword option.  For each block of elements add one card to the 
deck.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BBEG 
BEND 
INCR 
Type 
I 
I 
I 
Generalized  Beam  Element  Range  Cards.    This  Card  2  format  applies  to  the 
GENERAL keyword option.  Include as many cards as needed.  This input ends at the 
next keyword (“*”) card.  
Card 2… 
1 
Variable 
OPTION 
Type 
A 
2 
E1 
I 
3 
E2 
I 
4 
E3 
I 
5 
E4 
I 
6 
E5 
I 
7 
E6 
I 
8 
E7 
I 
  VARIABLE   
DESCRIPTION
SID 
K1 
K2 
⋮ 
Set ID 
First beam element 
Second beam element 
⋮  
B[N]BEG 
First beam element ID in block N.
B[N]END 
BBEG 
BEND 
INCR 
*SET 
DESCRIPTION
Last beam element ID in block N.  All defined ID’s between and
including B[N]BEG to B[N]END are added to the set.  These sets 
are  generated  after  all  input  is  read  so  that  gaps  in  the  element
numbering  are  not  a  problem.    B[N]BEG  and  B[N]END  may 
simply be limits on the ID’s and not element ID’s. 
First beam element ID in block. 
Last beam element ID in block.   
Beam ID increment.  Beam IDs BBEG, BBEG + INCR, BBEG + 2 ×
INCR,  and so on through BEND are added to the set. 
OPTION 
Option for GENERAL.  See table below. 
E1, …, E7 
Specified  entity.    Each  card  must  have  the  option  specified.    See
table below. 
The General Option: 
The  “OPTION”  column  in  the  table  below  enumerates  the  allowed  values  for  the 
“OPTION” variable in Card 2 for the GENERAL option.  Likewise, the variables E1, …, 
E7 refer to the GENERAL option Card 2. 
Each  of  the  following  operations  accept  up  to  7  arguments,  but  they  may  take  fewer.  
Values of “En” left unspecified are ignored. 
OPTION 
ALL 
ELEM 
DESCRIPTION 
All beam elements will be included in the set. 
Elements E1, E2, E3, ...  will be included. 
DELEM 
Elements E1, E2, E3, ...  previously added will be excluded. 
PART 
Elements of parts E1, E2, E3, ...  will be included. 
DPART 
BOX 
DBOX 
Elements  of  parts  E1,  E2,  E3,  ...    previously  added  will  be
excluded. 
Elements inside boxes E1, E2, E3, ...  will be included.   
Elements  inside  boxes  E1,  E2,  E3,  ...    previously  added  will  be
excluded.
*SET_BEAM_ADD 
Purpose:  Define a beam set by combining beam sets. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
Type 
I 
Default 
none 
Beam Element Set Cards.  Each card can be used to specify up to 8 beam element sets. 
Include as many cards of this kind as necessary.  This input ends at the next keyword 
(“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BSID1 
BSID2 
BSID3 
BSID4 
BSID5 
BSID6 
BSID7 
BSID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
SID 
DESCRIPTION
Set ID of new beam set.  All beam sets should have a unique set
ID. 
BSID[N] 
The Nth beam set ID on the card
*SET 
Purpose:    Define  a  beam  set  as  the  intersection,  ∩,  of  a  series  of  beam  sets.    The  new 
beam set, SID, contains only the elements common to of all beam sets listed on the cards 
of format 2. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
Type 
I 
Default 
none 
Beam Set Cards.  Each card can be used to specify up to 8 beam sets.  Include as many 
cards of this kind as necessary.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BSID1 
BSID2 
BSID3 
BSID4 
BSID5 
BSID6 
BSID7 
BSID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
SID 
DESCRIPTION
Set ID of new beam set.  All beam sets should have a unique set
ID. 
BSID[N] 
The Nth beam set ID on card2
*SET_BOX 
Purpose:  Define a set of boxes.  The new box set, SID, contains a set of box IDs listed on 
the cards of format 2.  Refer box ID in *DEFINE_BOX. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
Type 
I 
Default 
none 
Box  Set  Cards.    Each  card  can  be  used  to  specify  up  to  8  box  IDs.    Include  as  many 
cards of this kind as necessary.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BID1 
BID2 
BID3 
BID4 
BID5 
BID6 
BID7 
BID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
SID 
Set ID of new box set.  All box sets should have a unique set ID. 
BID[N] 
The Nth box ID on card2
*SET_DISCRETE_{OPTION1}_{OPTION2} 
For OPTION1 the available options are: 
<BLANK> 
GENERATE 
GENERAL 
For OPTION2 the available option is: 
COLLECT 
The option GENERATE will generate a block of discrete element ID’s between a starting 
ID and an ending ID.  An arbitrary number of blocks can be specified to define the set. 
Purpose:  Define a set of discrete elements. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
Type 
I 
Default 
none 
Discrete  Element  ID  Cards.    This  Card  2  format  applies  to  the  case  of  an  unset 
(<BLANK>)  keyword  option.    Set  one  value  per  element  in  the  set.    Include  as  many 
cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 2 
Variable 
1 
K1 
Type 
I 
2 
K2 
I 
3 
K3 
I 
4 
K4 
I 
5 
K5 
I 
6 
K6 
I 
7 
K7 
I 
8 
K8
Discrete  Element  Range  Cards.    This  Card  2  format  applies  to  the  GENERATE 
keyword  option.    Set  one  pair  of  BNBEG  and  BNEND  values  per  block  of  elements. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
B1BEG 
B1END 
B2BEG 
B2END 
B3BEG 
B3END 
B4BEG 
B4END 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Generalized  Discrete  Element  Range  Cards.    This  Card  2  format  applies  to  the 
GENERAL keyword option.  Include as many cards as needed.  This input ends at the 
next keyword (“*”) card.  
  Card 2 
1 
Variable 
OPTION 
Type 
A 
2 
E1 
I 
3 
E2 
I 
4 
E3 
I 
5 
E4 
I 
6 
E5 
I 
7 
E6 
I 
8 
E7 
I 
  VARIABLE   
DESCRIPTION
SID 
K1 
K2 
⋮ 
Set ID 
First discrete element 
Second discrete element 
⋮  
B[N]BEG 
First discrete element ID in block N. 
B[N]END 
Last  discrete  element  ID  in  block  N.    All  defined  ID’s  between
and including B[N]BEG to B[N]END are added to the set.  These 
sets  are  generated  after  all  input  is  read  so  that  gaps  in  the
element  numbering  are  not  a  problem.    B[N]BEG  and  B[N]END 
may simply be limits on the ID’s and not element ID’s. 
OPTION 
Option for GENERAL.  See table below. 
E1, …, E7 
Specified  entity.    Each  card  must  have  the  option  specified.    See
table below.
*SET 
The  “OPTION”  column  in  the  table  below  enumerates  the  allowed  values  for  the 
“OPTION” variable in Card 2 for the GENERAL option.  Likewise, the variables E1, …, 
E7 refer to the GENERAL option Card 2. 
Each  of  the  following  operations  accept  up  to  7  arguments,  but  they  may  take  fewer.  
Values of “En” left unspecified are ignored. 
OPTION 
ALL 
ELEM 
DESCRIPTION 
All discrete elements will be included in the set. 
Elements E1, E2, E3, ...  will be included. 
DELEM 
Elements E1, E2, E3, ...  previously added will be excluded. 
PART 
Elements of parts E1, E2, E3, ...  will be included. 
DPART 
BOX 
DBOX 
Elements  of  parts  E1,  E2,  E3,  ...    previously  added  will  be
excluded. 
Elements  inside  boxes  E1,  E2,  E3,  ...    will  be  included.     
Elements  inside  boxes  E1,  E2,  E3,  ...    previously  added  will  be 
excluded.
*SET_DISCRETE_ADD 
Purpose:  Define a discrete set by combining discrete sets.   
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
Type 
I 
Default 
none 
Discrete  Element  Set  Cards.    Each  card  can  be  used  to  specify  up  to  8  discrete 
element sets.  Include as many cards of this kind as necessary.  This input ends at the 
next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DSID1 
DSID2 
DSID3 
DSID4 
DSID5 
DSID6 
DSID7 
DSID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
SID 
DESCRIPTION
Set ID of new discrete element set.  All discrete element sets must
have a unique ID. 
DSID[N] 
The Nth discrete set ID on card2
Available options include: 
<BLANK> 
LIST 
LIST_GENERATE 
*SET 
The  last  option,  LIST_GENERATE,  will  generate  a  block  of  mode  ID’s  between  a 
starting ID and an ending ID.  An arbitrary number of blocks can be specified to define 
the set. 
Purpose:  Define a set of modes. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
Type 
I 
Default 
none 
Mode ID Cards.  This Card 2 format applies to the for keyword option set to LIST or
for an unset (<BLANK>) keyword option.  Set one value per mode in the set.  Include 
as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID1 
MID2 
MID3 
MID4 
MID5 
MID6 
MID7 
MID8 
Type 
I 
I 
I 
I 
I 
I 
I
Mode Range Cards.  This Card 2 format applies to the GENERATE keyword option. 
Set one pair of BNBEG and BNEND values per block of modes.  Include as many cards 
as needed.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  M1BEG  M1END  M2BEG  M2END  M3BEG  M3END  M4BEG  M4END 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
SID 
Set identification.  All mode sets should have a unique set ID. 
MID[N] 
Mode ID N. 
M[N]BEG 
First mode ID in block N. 
M[N]END 
Last mode ID in block N.  All defined ID’s between and including
M[N]BEG and M[N]END are added to the set. 
Remarks: 
1.  The available mode ID’s can be found in ASCII file eigout, or binary database 
d3eigv.
*SET_MULTI 
Note that this keyword’s name has been shortened.  Its older long form, however, is still 
also valid. 
*SET_MULTI-MATERIAL_GROUP_LIST 
Purpose:    This  command  defines  an  ALE  multi-material  set  ID  (AMMSID)  which 
contains a collection of one or more ALE multi-material group ID(s) (AMMGID).  This 
provides  a  means  for  selecting  any  specific  ALE  multi-material(s).    Application 
includes,  for  example,  a  selection  of  any  particular  fluid(s)  to  be  coupled  to  a  fluid-
structure interaction. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
AMSID 
Type 
Default 
I 
0 
Multi-Material Group ID Cards.  Set one value per element in the set.  Include as many 
cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
AMGID1 
AMGID2 
AMGID3 
AMGID4 
AMGID5 
AMGID6 
AMGID7 
AMGID8 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
  VARIABLE   
AMSID 
DESCRIPTION
An  ALE  multi-material  set  ID  (AMSID)  which  contains  a
collection  of  one  or  more  ALE  multi-material  group  ID(s) 
(AMGID). 
AMGID1 
The 1st ALE multi-material group ID (AMGID = 1) defined by the 
1st data line of the *ALE_MULTI-MATERIAL_GROUP card. 
⋮ 
⋮
*SET_MULTI-MATERIAL_GROUP_LIST 
DESCRIPTION
The  8th  ALE  multi-material  group  ID  (AMGID = 1)  defined  by 
the 8th data line of the *ALE_MULTI-MATERIAL_GROUP card. 
*SET 
  VARIABLE   
AMGID8 
Remarks: 
1.  Refer to an example in the *CONSTRAINED_LAGRANGE_IN_SOLID section.
*SET_NODE_{OPTION1}_{OPTION2} 
For OPTION1 the available options are: 
<BLANK> 
LIST 
COLUMN 
LIST_GENERATE 
LIST_GENERATE_INCREMENT 
GENERAL 
LIST_SMOOTH 
For OPTION2 the available option is: 
COLLECT 
The LIST option generates a set for a list of node IDs.  The LIST_GENERATE and LIST_-
GENERATE_INCREMENT  options  will  generate  block(s)  of  node  IDs  between  a 
starting ID and an ending ID.  An arbitrary number of blocks can be specified to define 
the node set.  The option LIST_SMOOTH is used to define a local region on a distorted 
tooling mesh to be smoothed.  The LIST_SMOOTH option is documented in the Local 
smoothing  of  tooling  mesh  section  of  the  *INTERFACE_COMPENSATION_NEW 
card’s documentation.  The COLUMN option is for setting nodal attributes, which pass 
data to other keyword cards, on a node-by-node basis. 
Purpose:  Define a nodal set with some identical or unique attributes. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
DA1 
DA2 
DA3 
DA4 
SOLVER 
Type 
I 
F 
Default 
none 
0. 
Remark 
1 
F 
0. 
1 
F 
0. 
1 
F 
A 
0. 
MECH 
1
Node  ID  Cards.    This  Card  2  format  applies  to  LIST  and  LIST_SMOOTH  keyword 
options.    Additionally,  it  applies  to  the  case  of  an  unset  (<BLANK>)  keyword option. 
Set one value per node in the set.  Include as many cards as needed.  This input ends at 
the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID1 
NID2 
NID3 
NID4 
NID5 
NID6 
NID7 
NID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Node ID with Column Cards.  This Card 2 format applies to the COLUMN keyword 
option.  Include one card per node in the set.  Include as many cards as needed.  This 
input ends at the next keyword (“*”) card. 
  Card 2 
1 
Variable 
NID 
Type 
I 
Remark 
2 
A1 
F 
2 
3 
A2 
F 
2 
4 
A3 
F 
2 
5 
A4 
F 
2 
6 
7 
8 
Node ID Range Cards.  This Card 2 format applies to the LIST_GENERATE keyword 
option.    Set  one  pair  of  BNBEG  and  BNEND  values  per  block  of  nodes.    Include  as 
many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
B1BEG 
B1END 
B2BEG 
B2END 
B3BEG 
B3END 
B4BEG 
B4END 
Type 
I 
I 
I 
I 
I 
I 
I
Node ID Range with Increment Cards.  This Card 2 format applies to the LIST_GEN-
ERATE_INCREMENT  keyword  option.    For  each  block  of  nodes  add  one  card  to  the 
deck.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BBEG 
BEND 
INCR 
Type 
I 
I 
I 
Generalized  Node  ID  Range  Cards.    This  Card  2  format  applies  to  the  GENERAL 
keyword  option.    Include  as  many  cards  as  needed.    This  input  ends  at  the  next 
keyword (“*”) card.  
  Card 2 
1 
Variable 
OPTION 
Type 
A 
2 
E1 
I 
3 
E2 
I 
4 
E3 
I 
5 
E4 
I 
6 
E5 
I 
7 
E6 
I 
8 
E7 
I 
  VARIABLE   
DESCRIPTION
SID 
DA1 
DA2 
DA3 
DA4 
Set identification.  All node sets should have a unique set ID. 
First nodal attribute default value, see remark 1 below. 
Second nodal attribute default value 
Third nodal attribute default value 
Fourth nodal attribute default value 
SOLVER 
Name of solver using this set (MECH, CESE, etc.) 
NIDi 
NID 
A1 
A2 
A3 
A4 
Node ID i 
Nodal ID 
First nodal attribute, see remark 2 below. 
Second nodal attribute 
Third nodal attribute 
Fourth nodal attribute
VARIABLE   
DESCRIPTION
BnBEG 
First node ID in block n. 
BnEND 
BBEG 
BEND 
INCR 
Last node ID in block n.  All defined ID’s between and including 
BnBEG to BnEND are added to the set.  These sets are generated
after all input is read so that gaps in the node numbering are not a
problem.    BnBEG  and  BnEND  may  simply  be  limits  on  the  ID’s 
and not nodal ID’s. 
First node ID in block. 
Last node ID in block.   
Node ID increment.  Node IDs BBEG, BBEG + INCR, BBEG + 2 ×
INCR,  and so on through BEND are added to the set. 
OPTION 
Option for GENERAL.  See table below. 
E1, …, E7 
Specified  entity.    Each  card  must  have  the  option  specified.    See 
table below. 
The General Option: 
The  “OPTION”  column  in  the  table  below  enumerates  the  allowed  values  for  the 
“OPTION” variable in Card 2 for the GENERAL option.  Likewise, the variables E1, …, 
E7 refer to the GENERAL option Card 2. 
Each  of  the  following  operations  accept  up  to  7  arguments,  but  they  may  take  fewer.  
Values of “En” left unspecified are ignored. 
OPTION 
DESCRIPTION 
ALL 
All nodes will be included in the set. 
NODE 
Nodes E1, E2, E3, … will be included. 
DNODE 
Nodes E1, E2, E3, … previously added will be excluded. 
PART 
Nodes of parts E1, E2, E3, … will be included. 
DPART 
Nodes of parts E1, E2, E3, … previously added will be excluded. 
BOX 
Nodes  inside  boxes  E1,  E2,  E3,  …  will  be  included.
DBOX 
VOL 
DVOL 
SET_XXXX 
SALECPT 
*SET 
DESCRIPTION 
Nodes  inside  boxes  E1,  E2,  E3,  …  previously  added  will  be
excluded. 
Nodes  inside  contact  volumes  E1,  E2,  E3,  …  will  be  included.
 
Nodes  inside  contact  volumes  E1,  E2,  E3,  …  previously  added
will be excluded. 
Include  nodal  points  of  element  sets  defined  by  SET_XXXX_
LIST,  where  XXXX  could  be  SHELL,  SOLID,  BEAM,  TSHELL 
and SPRING 
Nodes inside a box in Structured ALE mesh.  E1 here is the S-ALE 
mesh  ID  (MSHID).    E2,  E3,  E4,  E5,  E6,  E7  correspond  to  XMIN,
XMAX,  YMIN,  YMAX,  ZMIN,  ZMAX.    They  are  the  minimum
and  the  maximum  nodal  indices  along  each  direction  in  S-ALE 
mesh.    This  option  is  only  to  be  used  for  Structured  ALE  mesh
and should not be used in a mixed manner with other “_GENER-
AL” options. 
refer 
Please 
*ALE_STRUCTURED_MESH_CONTROL_-
POINTS  and  *ALE_STRUCTURED_MESH_CONTROL  for  more 
details.   
to 
SALEFAC 
Nodes  that  are  on  the  face  of  a  Structured  ALE  mesh.    E1  gives
the S-ALE mesh ID (MSHID).  E2, E3, E4, E5, E6, E7 correspond to
-𝑥,  +𝑥,  -𝑦,  +𝑦,  -𝑧,  +𝑧  faces.    Assigning  1,  for  instance,  to  these  6 
values  would  include  all  the  surface  segments  at  these  faces  in
the  segment  set.    This  option  is  only  to  be  used  for  Structured
ALE mesh and should not be used in a mixed manner with other
“_GENERAL” options. 
refer 
*ALE_STRUCTURED_MESH_CONTROL_-
Please 
POINTS  and  *ALE_STRUCTURED_MESH_CONTROL  for  more 
details.   
to 
Remarks: 
1.  Nodal attributes can be assigned to pass data to other keywords.  For example, 
for  contact  option,  *CONTACT_TIEBREAK_NODES_TO_SURFACE  the  attrib-
utes are:
DA1  =  NFLF   ⇒  Normal failure force, 
  DA2  =  NSFL  ⇒  Shear failure force, 
  DA3  =  NNEN  ⇒  Exponent for normal force, 
  DA4  =  NMES  ⇒  Exponent for shear force. 
2.  The  default  nodal  attributes  can  be  overridden  on  these  cards;  otherwise, 
A1 = DA1, etc. 
3.  This  field  is  used  by  a  non-mechanics  solver  to  create  a  set  defined  on  that 
solver’s mesh.  By default, the set refers to the mechanics mesh.  
4.  The  option  *SET_NODE_LIST_SMOOTH  is  used  for  localized  tooling  surface 
smoothing,  and  is  used  in  conjunction  with  keywords  *INTERFACE_COM-
PENSATION_NEW_LOCAL_SMOOTH, 
*INCLUDE_COMPENSATION_-
ORIGINAL_RIGID_TOOL, and *INCLUDE_COMPENSATION_NEW_RIGID_-
TOOL.  This option is available in R6 Revision 73850 and later releases
Available options include: 
<BLANK> 
ADVANCED 
*SET 
Purpose:  Define a node set by combining node sets or for the ADVANCED option by 
combining, NODE, SHELL, SOLID, BEAM, SEGMENT, DISCRETE and THICK SHELL 
sets. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSID 
DA1 
DA2 
DA3 
DA4 
SOLVER 
Type 
I 
F 
F 
F 
F 
A 
Default 
none 
none 
none 
none 
none  MECH 
Remark 
1 
Node  Set  Cards.    This  Card  2  format  is  used  when  the  keyword  option  is  left  unset 
(<BLANK>).  Each card can be used to specify up to 8 node set IDs.  Include as many 
cards of this kind as necessary.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSID1 
NSID2 
NSID3 
NSID4 
NSID5 
NSID6 
NSID7 
NSID8 
Type 
I 
I 
I 
I 
I 
I 
I
Node Set Advanced Cards.  This Card 2 format is used when the keyword option is 
set to ADVANCED.  Each card can be used to specify up to 4 set IDs (node sets, beam 
sets,  etc…).    Include  as  many  cards  of  this  kind  as  necessary.    This  input  ends  at  the 
next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID1 
TYPE1 
SID2 
TYPE2 
SID3 
TYPE3 
SID4 
TYPE4 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
NSID 
DA1 
DA2 
DA3 
DA4 
Set  ID  of  new  node  set.    All  node  sets  should  have  a  unique  set
ID. 
First nodal attribute default value, see remark 1 below. 
Second nodal attribute default value 
Third nodal attribute default value 
Fourth nodal attribute default value 
SOLVER 
Name of solver using this set (MECH, CESE, etc.) 
NSID[N] 
The Nth node set ID on Card 2 in LIST format. 
SID[N] 
The Nth set ID on Card 2 in ADVANCED format. 
TYPE[N] 
Type set for SID[N]: 
EQ.1: Node set 
EQ.2: Shell set 
EQ.3: Beam set 
EQ.4: Solid set 
EQ.5: Segment set 
EQ.6: Discrete set 
EQ.7: Thick shell set
*SET 
1.  This  field  is  used  by  a  non-mechanics  solver  to  create  a  set  defined  on  that 
solver’s mesh.  By default, the set refers to the mechanics mesh.
*SET_NODE_INTERSECT 
Purpose:  Define a node set as the intersection, ∩, of a series of node sets.  The new node 
set, NSID, contains all common elements of all node sets listed on all cards in format 2. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
DA1 
DA2 
DA3 
DA4 
SOLVER 
Type 
I 
F 
F 
F 
F 
A 
Default 
none 
none 
none 
none 
none  MECH 
Remark 
1 
Node Set Cards.  For each SID in the intersection specify one field.  Include as many 
cards as necessary.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSID1 
NSID2 
NSID3 
NSID4 
NSID5 
NSID6 
NSID7 
NSID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
SID 
DESCRIPTION
Set  ID  of  new  node  set.    All  node  sets  should  have  a  unique  set
ID. 
DAi 
Nodal attribute of the i’th node. 
SOLVER 
Name of solver using this set (MECH, CESE, etc.) 
NSIDn 
The nth node set ID. 
Remarks: 
1.  This  field  is  used  by  a  non-mechanics  solver  to  create  a  set  defined  on  that 
solver’s mesh.  By default, the set refers to the mechanics mesh.
*SET_PART_{OPTION1}_{OPTION2}  
For OPTION1 available options are: 
<BLANK> 
LIST 
COLUMN 
LIST_GENERATE 
LIST_GENERATE_INCREMENT 
For OPTION2 the available option is: 
COLLECT 
The  LIST_GENERATE  and  LIST_GENERATE_INCREMENT  options  will  generate 
block(s)  of  part  IDs  between  a  starting  ID  and  an  ending  ID.    An  arbitrary  number  of 
blocks can be specified to define the part set. 
Purpose:    Define  a  set  of  parts  with  optional  attributes.    For  the  column  option,  see 
*AIRBAG or *CONSTRAINED_RIGID_BODY_STOPPERS. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
DA1 
DA2 
DA3 
DA4 
SOLVER 
Type 
I 
F 
F 
F 
F 
A 
Default 
none 
0. 
MECH 
Remark 
1 
1 
1 
1
Part ID Cards.  This Card 2 format applies to the LIST keyword option.  Additionally, 
it applies to the case of an unset (<BLANK>) keyword option.  Set one value per part in 
the  set.   Include  as  many  cards  as  needed.  This  input  ends  at  the  next keyword  (“*”) 
card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID1 
PID2 
PID3 
PID4 
PID5 
PID6 
PID7 
PID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Part  ID  with  Column  Cards.    This  Card  2  format  applies  to  the  COLUMN  keyword 
option.    Include  one  card  per  part  in  the  set.    Include  as  many  cards  as  needed.    This 
input ends at the next keyword (“*”) card. 
  Card 2 
1 
Variable 
PID 
Type 
I 
Remark 
2 
A1 
F 
2 
3 
A2 
F 
2 
4 
A3 
F 
2 
5 
A4 
F 
2 
6 
7 
8 
Part ID Range Cards.  This Card 2 format applies to the GENERATE keyword option. 
Set  one  pair  of  BNBEG  and  BNEND  values  per  block  of  part  IDs.    Include  as  many 
cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
B1BEG 
B1END 
B2BEG 
B2END 
B3BEG 
B3END 
B4BEG 
B4END 
Type 
I 
I 
I 
I 
I 
I 
I
Part ID Range with Increment Cards.  This Card 2 format applies to the LIST_GEN-
ERATE_INCREMENT  keyword  option.    For  each  block  of  parts  add  one  card  to  the 
deck.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BBEG 
BEND 
INCR 
Type 
I 
I 
I 
  VARIABLE   
DESCRIPTION
SID 
DA1 
DA2 
DA3 
DA4 
Set ID.  All part sets should have a unique set ID. 
First attribute default value, see remark 1 below. 
Second attribute default value 
Third attribute default value 
Fourth attribute default value 
SOLVER 
Name of solver using this set (MECH, CESE, etc.) 
PID 
PID1 
PID2 
⋮ 
A1 
A2 
A3 
A4 
Part ID 
First part ID 
Second part ID 
⋮  
First part attribute, see remark 2 below. 
Second part attribute 
Third part attribute 
Fourth part attribute 
B[N]BEG 
First part ID in block N. 
B[N]END 
Last part ID in block N.  All defined ID’s between and including
B[N]BEG  to  B[N]END  are  added  to  the  set.    These  sets  are 
generated  after  all  input  is  read  so  that  gaps  in  the  part
numbering  are  not  a  problem.    B[N]BEG  and  B[N]END  may 
simply be limits on the ID’s and not part ID’s.
VARIABLE   
DESCRIPTION
First part ID in block. 
Last part ID in block.   
Part  ID  increment.    Part  IDs  BBEG,  BBEG+INCR,  BBEG  +  2 × 
INCR,  and so on through BEND are added to the set. 
BBEG 
BEND 
INCR 
Remarks: 
1.  Part attributes can be assigned for some input types.  For example, for airbags a 
time delay, DA1 = T1, can be defined before pressure begins to act along with a 
time delay, DA2 = T2, before full pressure is applied, (default T2 = T1), and for 
the  constraint  option,  *CONSTRAINED_RIGID_BODY_STOPPERS  one  attrib-
ute  can  be  defined:  DA1,  the  closure  distance  which  activates  the  stopper  con-
straint. 
2.  The  default  part  attributes  can  be  overridden  on  the  part  cards;  otherwise, 
A1 = DA1, etc. 
3.  This  field  is  used  by  a  non-mechanics  solver  to  create  a  set  defined  on  that 
solver’s mesh.  By default, the set refers to the mechanics mesh.
Purpose:  Define a part set by combining part sets. 
*SET 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
DA1 
DA2 
DA3 
DA4 
SOLVER 
Type 
I 
F 
F 
F 
F 
A 
Default 
none 
MECH 
Remark 
1,2 
1,2 
1,2 
1,2 
3 
Part Set Cards.  Each card can be used to specify up to 8 part set IDs.  Include as many 
cards of this kind as necessary.  This input ends at the next keyword (“*”) card. 
Card 2… 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PSID1 
PSID2 
PSID3 
PSID4 
PSID5 
PSID6 
PSID7 
PSID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
SID 
DA1 
DA2 
DA3 
DA4 
Set ID.  All part sets should have a unique set ID. 
First attribute default value, see Remarks 1 and 2 below. 
Second attribute default value 
Third attribute default value 
Fourth attribute default value 
SOLVER 
Name of solver using this set (MECH, CESE, etc.)
VARIABLE   
DESCRIPTION
PSID[N] 
The Nth part set ID 
GT.0: PSIDn is added to SID, 
LT.0:  all  part  sets  with  ID  between  PSID(i-1)  and  |PSIDi|, 
including  PSID(i-1)  and  |PSIDi|,  will  be  added  to  SID. 
PSID(i-1)  has  to  be > 0  and  has  a  magnitude  smaller  or 
equal to |PSIDi | when PSIDi < 0. 
Remarks: 
1.  Part attributes can be assigned for some input types.  For example, for airbags a 
time delay, DA1 = T1, can be defined before pressure begins to act along with a 
time delay, DA2 = T2, before full pressure is applied, (default T2 = T1), and for 
the  constraint  option,  *CONSTRAINED_RIGID_BODY_STOPPERS  one  attrib-
ute  can  be  defined:  DA1,  the  closure  distance  which  activates  the  stopper  con-
straint. 
2.  The default values  for the part attributes are given in the contributing  *SET_-
PART_{OPTION}  commands.    Nonzero  values  of  DA1,  DA2,  DA3,  or  DA4  in 
*SET_PART_ADD will override the respective default values. 
3.  This  field  is  used  by  a  non-mechanics  solver  to  create  a  set  defined  on  that 
solver’s mesh.  By default, the set refers to the mechanics mesh.
*SET_SEGMENT_{OPTION1}_{OPTION2} 
For OPTION1 the available options are: 
<BLANK> 
GENERAL 
For OPTION2  the available option is  
COLLECT 
Purpose:  Define set of segments with optional identical or unique attributes.  For three-
dimensional  geometries,  a  segment  can  be  triangular  or  quadrilateral.    For  two-
dimensional  geometries,  a  segment  is  a  line  defined  by  two  nodes  and  the  GENERAL 
option does not apply. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
DA1 
DA2 
DA3 
DA4 
SOLVER 
Type 
I 
F 
Default 
none 
0. 
Remarks 
1 
F 
0. 
1 
F 
0. 
1 
F 
A 
0. 
MECH 
1 
4 
Segment  Cards.    For  each  segment  in  the  set  include  on  card  of  this  format.    Set 
N3 = N4 for triangular segments.  Include as many cards as necessary.  This input ends 
at the next keyword (“*”) card. 
  Card 2 
Variable 
1 
N1 
Type 
I 
2 
N2 
I 
3 
N3 
I 
Remarks 
4 
N4 
I 
2 
5 
A1 
F 
3 
6 
A2 
F 
3 
7 
A3 
F 
3 
8 
A4 
F
Generalized  Part  ID  Range  Cards.    This  Card  2  format  applies  to  the  GENERAL 
keyword  option.    Include  as  many  cards  as  needed.    This  input  ends  at  the  next 
keyword (“*”) card.  
  Card 2 
1 
Variable 
OPTION 
Type 
A 
2 
E1 
I 
3 
E2 
I 
4 
E3 
5 
E4 
6 
E5 
7 
E6 
8 
E7 
I 
I or F 
I or F 
I or F 
I or F 
  VARIABLE   
DESCRIPTION
SID 
DA1 
DA2 
DA3 
DA4 
Set ID.  All segment sets should have a unique set ID. 
First segment attribute default value, see remark 1 below. 
Second segment attribute default value 
Third segment attribute default value 
Fourth segment attribute default value 
SOLVER 
Name of solver using this set (MECH, CESE, etc.) 
N1 
N2 
N3 
N4 
A1 
A2 
A3 
A4 
NFLS 
SFLS 
Nodal point 𝑛1 
Nodal point 𝑛2 
Nodal point 𝑛3 
Nodal point 𝑛4, see Remark 2 below. 
First segment attribute, see Remark 3 below. 
Second segment attribute 
Third segment attribute 
Fourth segment attribute 
Normal failure stress 
Shear failure stress.  Failure criterion: 
OPTION 
Option for GENERAL.  See table below.
E1, …, E7 
DESCRIPTION
Specified  entity.    Each  card  must  have  an  option  specified.    See
table below. 
*SET 
The General Option: 
The  “OPTION”  column  in  the  table  below  enumerates  the  allowed  values  for  the 
“OPTION” variable in Card 2 for the GENERAL option.  Likewise, the variables E1, …, 
E7 refer to the GENERAL option Card 2. 
Each  of  the  following  operations  accept  up  to  7  arguments,  but  they  may  take  fewer.  
Values of “En” left unspecified are ignored. 
OPTION 
DESCRIPTION 
ALL 
BOX 
BOX_SHELL 
BOX_SLDIO 
BOX_SOLID 
PART 
All exterior segments will be included in the set. 
Generate segments inside boxes having IDs E1, E2, and E3 with 
attributes having values E4, E5, E6, and E7.  For shell elements 
one segment per shell is generated.  For solid elements only those 
segments wrapping the solid part and pointing outward from the 
part will be generated. 
Generate segments inside boxes having IDs E1, E2, and E3 with 
attributes having values E4, E5, E6, and E7.  The segments are 
only generated for shell elements.  One segment per shell is 
generated. 
Generate segments inside boxes having IDs E1, E2, and E3 with 
attributes having values E4, E5, E6, and E7.  Both exterior 
segments and inter-element segments are generated. 
Generate segments inside boxes having IDs E1, E2, and E3 with 
attributes having values E4, E5, E6, and E7.  The segments are 
only generated for exterior solid elements 
Generate segments of parts E1, E2, and E3 with attributes E4, E5, 
E6, and E7.  For shell elements one segment per shell is 
generated.  For solid elements only those segments wrapping the 
solid part and pointing outward from the part will be generated.  
PART could refer to beam parts when defining 2D segments for 
traction application.
DESCRIPTION 
*SET_SEGMENT 
PART_IO 
PSLDFi 
SEG 
VOL 
Generate segments from parts E1, E2, E3 with attributes E4, E5, 
E6, and E7.  Same as the PART option above except that inter-
element segments inside parts will be generated as well.  This 
option is sometimes useful for single surface contact of solid 
elements to prevent negative volumes. 
Generate segments from the i’th face of solid parts E1, E2, E3 with 
attributes E4, E5, E6, and E7.  See table below for face definition. 
Create segment with node IDs E1, E2, E3, and E4. 
Generate segments inside contact volume IDs E1, E2, and E3 with 
attributes having values E4, E5, E6, and E7.  See BOX option for 
other details. 
VOL_SHELL 
Generate segments for shells inside contact volume IDs E1, E2, 
and E3 with attributes having values E4, E5, E6, and E7 
VOL_SLDIO 
VOL_SOLID 
Generate segments for solid elements inside contact volume IDs 
E1, E2, and E3 with attributes E4, E5, E6, and E7.  See BOX_-
SLDIO for other details. 
Generate segments for solid elements inside contact volume IDs 
E1, E2, and E3 with attributes E4, E5, E6, and E7.  See BOX_SOL-
ID for other details. 
SET_SHELL 
Generate segments for shell elements in SET_SHELL_LIST with 
IDs E1, E2, and E3 with attributes E4, E5, E6, and E7. 
SET_SOLID 
SET_SLDIO 
SET_SLDFi 
Generate segments for solid elements in SET_SOLID_LIST with 
IDs E1, E2, and E3 with attributes E4, E5, E6, and E7. 
Generate segments for solid elements in SET_SOLID_LIST with 
IDs E1, E2, and E3 with attributes E4, E5, E6, and E7.  Both 
exterior & interior segments are generated. 
Generate segments from the ith face of solid elements in SET_-
SOLID_LIST with IDs E1, E2, and E3 with attributes E4, E5, E6, 
and E7.  See table below for face definition. 
SET_TSHELL 
Generate segments for thick shell elements in SET_TSHELL_LIST 
with IDs of E1, E2, and E3 with attributes E4, E5, E6, and E7.  
Only exterior segments are generated.
DESCRIPTION 
*SET 
SET_TSHIO 
Generate segments for thick shell elements in SET_TSHELL_LIST 
with IDs of E1, E2, and E3 with attributes E5, E5, E6, and E7.  
Both exterior & interior segments are generated. 
DBOX 
Segments inside boxes with IDs E1, …, E7 will be excluded. 
DBOX_SHELL 
Shell related segments inside boxes of IDs E1, …, E7 will be 
excluded. 
DBOX_SOLID 
Solid related segments inside boxes of IDs E1, …, E7 will be 
excluded. 
DPART 
Segments of parts with IDs E1, …, E7 will be excluded. 
DSEG 
DVOL 
Segment with node IDs  E1, E2, E3, and E4 will be deleted. 
Segments inside contact volumes having IDs E1, …, E7 will be 
excluded. 
DVOL_SHELL 
Shell related segments inside contact volumes having IDs E1, …, 
E7 will be excluded. 
DVOL_SOLID 
Solid related segments inside contact volumes having IDs E1, …, 
E7 will be excluded. 
SALECPT 
Segments inside a box in Structured ALE mesh.  E1 here is the S-
ALE mesh ID (MSHID).  E2, E3, E4, E5, E6, E7 correspond to 
XMIN, XMAX, YMIN, YMAX, ZMIN, ZMAX.  They are the 
minimum and the maximum nodal indices along each direction 
in S-ALE mesh.  This option is only to be used for Structured ALE 
mesh and should not be used in a mixed manner with other 
“_GENERAL” options.    
Please refer to *ALE_STRUCTURED_MESH_CONTROL_-
POINTS and *ALE_STRUCTURED_MESH_CONTROL for more 
details.
DESCRIPTION 
*SET_SEGMENT 
Segments on the face of Structured ALE mesh.  E1 here is the S-
ALE mesh ID (MSHID).  E2, E3, E4, E5, E6, E7 correspond to -X, 
+X, -Y, +Y, -Z, +Z faces.  Assigning 1 to these 6 values would 
include all the surface segments at these faces in the segment set.  
This option is only to be used for Structured ALE mesh and 
should not be used in a mixed manner with other “_GENERAL” 
options. 
Please refer to *ALE_STRUCTURED_MESH_CONTROL_-
POINTS and *ALE_STRUCTURED_MESH_CONTROL for more 
details.   
SALEFAC 
Remarks: 
1.  Segment attributes can be assigned for some input types.  For example, for the 
contact options. 
The attributes for the SLAVE surface are: 
DA1 (NFLS)  =  Normal  failure  stress,  *CONTACT_TIEBREAK_SURFACE 
contact only, 
DA2 (SFLS)  =  Shear  failure  stress,  *CONTACT_TIEBREAK_SURFACE 
contact only, 
DA3 (FSF)  =  Coulomb friction scale factor, 
DA4 (VSF)  =  Viscous friction scale factor, 
and the attributes for the MASTER surface are: 
DA3 (FSF)  =  Coulomb friction scale factor, 
DA4 (VSF)  =  Viscous friction scale factor. 
For airbags, see *AIRBAG, a time delay, DA1 = T1, can be defined before pres-
sure begins to act on a segment along with a time delay, DA2 = T2, before full 
pressure  is  applied  to  the  segment,  (default  T2 = T1),  and  for  the  constraint 
option, 
2.  To define a triangular segment make N4 equal to N3. 
3.  The  default  segment  attributes  can  be  overridden  on  these  cards,  otherwise, 
A1 = DA1, A2 = DA2, etc. 
4.  This  field  is  used  by  a  non-mechanics  solver  to  create  a  set  defined  on  that 
solver’s mesh.  By default, the set refers to the mechanics mesh.
FACE 
Hexahedron 
Pentahedron 
Tetrahedron 
1 
2 
3 
4 
5 
6 
N1, N5, N8, N4 
N2, N3, N7, N6 
N1, N2, N6, N5 
N4, N8, N7, N3 
N1, N2, N5 
N1, N2, N4 
N4, N6, N3 
N2, N3, N4 
N1, N4, N3, N2 
N1, N3, N2 
N2, N3, N6, N5 
N1, N4, N3 
N1, N4, N3, N2 
N1, N5, N6, N4 
N5, N6, N7, N8 
Table 4.1  Face definition of solid elements
*SET_SEGMENT_ADD 
Purpose:  Define a segment set by combining segment sets.   
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
SOLVER 
Type 
I 
A 
Default 
none  MECH 
Remark 
1 
Segment  Set  Cards.    Each  card  can  be  used  to  specify  up  to  8  segment  set  IDs. 
Include as many cards of this kind as necessary.  This input ends at the next keyword 
(“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID1 
SSID2 
SSID3 
SSID4 
SSID5 
SSID6 
SSID7 
SSID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
SID 
DESCRIPTION
Set ID of new segment set.  All segment sets should have a unique
set ID. 
SOLVER 
Name of solver using this set (MECH, CESE, etc.) 
SSID[N] 
The Nth segment set ID on card2. 
Remarks: 
1.  This  field  is  used  by  a  non-mechanics  solver  to  create  a  set  defined  on  that 
solver’s mesh.  By default, the set refers to the mechanics mesh.
*SET 
Purpose:    Define  a  segment  set  as  the  intersection, ∩,  of  a  series of  segment  sets.    The 
new segment set, SID, contains all segments common to the sets listed on all of the cards 
in format 2. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
SOLVER 
Type 
I 
A 
Default 
none  MECH 
Remark 
1 
Segment  Set  Cards.    For  each  SID  in  the  intersection  specify  one  field.    Include  as 
many cards as necessary.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID1 
SSID2 
SSID3 
SSID4 
SSID5 
SSID6 
SSID7 
SSID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
SID 
DESCRIPTION
Set ID of new segment set.  All segment sets should have a unique
set ID. 
SOLVER 
Name of solver using this set (MECH, CESE, etc.) 
SSID[N] 
The Nth segment set ID 
Remarks: 
1.  This  field  is  used  by  a  non-mechanics  solver  to  create  a  set  defined  on  that 
solver’s mesh.  By default, the set refers to the mechanics mesh.
*SET_2D_SEGMENT_{OPTION1}_{OPTION2} 
For OPTION1 the available options are: 
<BLANK> 
SET 
For OPTION2 the available option is: 
COLLECT 
Purpose:    Define  a  set  of  boundary  line  segments  in  two-dimensional  axisymmetric, 
plane stress, and plane strain geometries with optional attributes.  This command does 
not  apply  to  beam  formulations  7  and  8.    It  is  sometimes  convenient  for  two-
dimensional  parts  which  are  subject  to  adaptivity  because  the  segments  in  the  set  are 
updated as the geometry adapts. 
Card  Sets.    For  each  set  include  a  pair  of  cards  1  and  2.    This  input  ends  at  the  next 
keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
DA1 
DA2 
DA3 
DA4 
F 
0. 
1 
3 
F 
0. 
1 
4 
F 
0. 
1 
5 
6 
7 
8 
Type 
I 
F 
Default 
none 
0. 
1 
2 
Remarks 
  Card 2 
1 
Variable 
PID/PSID 
Type 
Remarks 
I
VARIABLE   
DESCRIPTION
SID 
DA1 
DA2 
DA3 
DA4 
Set ID.  All segment sets should have a unique set ID. 
First segment attribute default value, see remark 1 below. 
Second segment attribute default value 
Third segment attribute default value 
Fourth segment attribute default value 
PID/PSID 
Part ID or part set ID if SET option is specified. 
Remarks: 
1.  The boundary along r = 0 isn’t included in axisymmetric problems. 
2.  The common boundary between parts in the part set PSID is not included in the 
boundary segments.
*SET_SHELL_{OPTION1}_{OPTION2} 
For OPTION1 the available options are: 
<BLANK> 
LIST   
COLUMN 
LIST_GENERATE 
LIST_GENERATE_INCREMENT 
GENERAL 
For OPTION2 the available option is: 
COLLECT 
The  LIST_GENERATE  and  LIST_GENERATE_INCREMENT  options  will  generate 
block(s)  of  shell  element  IDs  between  a  starting  ID  and  an  ending  ID.    An  arbitrary 
number of blocks can be specified to define the shell element set. 
Purpose:  Define a set of shell elements with optional identical or unique attributes. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
DA1 
DA2 
DA3 
DA4 
Type 
I 
F 
Default 
none 
0. 
Remarks 
1 
F 
0. 
1 
F 
0. 
1 
F 
0.
Shell  Element  ID  Cards.    This  Card  2  format  applies  to  LIST  keyword  option. 
Additionally,  it  applies  to  the  case  of  an  unset  (<BLANK>)  keyword  option.    Set  one 
value per element in the set.  Include as many cards as needed.  This input ends at the 
next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EID1 
EID2 
EID3 
EID4 
EID5 
EID6 
EID7 
EID8 
Type 
Remarks 
I 
2 
I 
2 
I 
2 
I 
2 
I 
2 
I 
2 
I 
2 
I 
2 
Shell  Element  ID  with  Column  Cards.    This  Card  2  format  applies  to  the  COLUMN 
keyword option.  Include one card per shell element in the set.  Include as many cards 
as needed.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
Variable 
EID 
Type 
I 
Remarks 
2 
A1 
F 
3 
3 
A2 
F 
3 
4 
A3 
F 
3 
5 
A4 
F 
3 
6 
7 
8 
Shell  Element  ID  Range  Cards.    This  Card  2  format  applies  to  the  GENERATE 
keyword option.  Set one pair of BNBEG and BNEND values per block of shell element 
IDs.  Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
B1BEG 
B1END 
B2BEG 
B2END 
B3BEG 
B3END 
B4BEG 
B4END 
Type 
I 
I 
I 
I 
I 
I 
I
Shell  Element  ID  Range  with  Increment  Cards.    This  Card  2  format  applies  to  the 
LIST_GENERATE_INCREMENT keyword option.  For each block of shell elements add 
one card to the deck.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BBEG 
BEND 
INCR 
Type 
I 
I 
I 
Generalized  Shell  Element  ID  Range  Cards.    This  Card  2  format  applies  to  the 
GENERAL keyword option.  Include as many cards as needed.  This input ends at the 
next keyword (“*”) card.  
  Card 2 
1 
Variable 
OPTION 
Type 
A 
2 
E1 
I 
3 
E2 
I 
4 
E3 
I 
5 
E4 
I 
6 
E5 
I 
7 
E6 
I 
8 
E7 
I 
  VARIABLE   
DESCRIPTION
SID 
DA1 
DA2 
DA3 
DA4 
EID1 
EID2 
⋮ 
EID 
A1 
A2 
A3 
Set ID.  All shell sets should have a unique set ID. 
First attribute default value, see remark 1. 
Second attribute default value 
Third attribute default value 
Fourth attribute default value 
First shell element ID, see remark 2. 
Second shell element ID 
⋮  
Element ID 
First attribute 
Second attribute 
Third attribute
DESCRIPTION
A4 
Fourth attribute 
BnBEG 
First shell ID in shell block n. 
*SET 
BnEND 
BBEG 
BEND 
INCR 
Last shell ID in block n.  All defined ID’s between and including 
BnBEG to BnEND are added to the set.  These sets are generated
after  all  input  is  read so  that  gaps  in the  element  numbering  are
not a problem.  BnBEG and BnEND may simply be limits on the 
ID’s and not element IDs. 
First shell element ID in block. 
Last shell element ID in block.   
Shell  element  ID  increment.    Shell  element  IDs  BBEG,  BBEG + 
INCR, BBEG + 2 × INCR,  and so on through BEND are added to
the set. 
OPTION 
Option for GENERAL.  See table below. 
E1, …, E7 
Specified  entity.    Each  card  must  have  the  option  specified.    See 
table below. 
The General Option: 
The  “OPTION”  column  in  the  table  below  enumerates  the  allowed  values  for  the 
“OPTION” variable in Card 2 for the GENERAL option.  Likewise, the variables E1, …, 
E7 refer to the GENERAL option Card 2. 
Each  of  the  following  operations  accept  up  to  7  arguments,  but  they  may  take  fewer.  
Values of “En” left unspecified are ignored. 
OPTION 
ALL 
ELEM 
DESCRIPTION 
All shell elements will be included in the set. 
Shell elements E1, E2, E3, … will be included. 
DELEM 
Shell elements E1, E2, E3, … previously added will be excluded. 
PART 
Shell elements of parts E1, E2, E3, … will be included. 
DPART 
Shell  elements  of  parts  E1,  E2,  E3,  …  previously  added  will  be
excluded.
BOX 
DBOX 
Remarks: 
*SET_SHELL 
DESCRIPTION 
Shell  elements  inside boxes  E1,  E2,  E3,  …  will  be  included.     
Shell  elements  inside  boxes E1,  E2,  E3,  …  previously  added  will
be excluded. 
1.  Shell attributes can be assigned for some input types. 
For example, for contact options, the attributes for the SLAVE surface are: 
DA1 (NFLS)  =  Normal  failure  stress,  *CONTACT_TIEBREAK_SURFACE 
contact only, 
DA2 (SFLS)  =  Shear  failure  stress,  *CONTACT_TIEBREAK_SURFACE 
contact only, 
DA3 (FSF)  =  Coulomb friction scale factor, 
DA4 (VSF)  =  Viscous friction scale factor, 
and the attributes for the MASTER surface are: 
DA1 (FSF)  =  Coulomb friction scale factor, 
DA2 (VSF)  =  Viscous friction scale factor. 
2.  The default attributes are taken. 
3.  The  default  shell  attributes  can  be  overridden  on  these  cards;  otherwise, 
A1 = DA1, etc.
Purpose:  Define a shell set by combining shell sets.   
*SET 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
Type 
I 
Default 
none 
Shell Element Set Cards.  Each card can be used to specify up to 8 shell element set 
IDs.    Include  as  many  cards  as  necessary.    This  input  ends  at  the  next  keyword  (“*”) 
card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID1 
SSID2 
SSID3 
SSID4 
SSID5 
SSID6 
SSID7 
SSID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
SID 
Set ID of new shell set.  All shell sets should have a unique set ID.
SSID[N] 
The Nth shell set ID on card2
*SET_SHELL_INTERSECT 
Purpose:  Define a shell set as the intersection, ∩, of a series of shell sets.  The new shell 
set, SID, contains all shells common to all sets on the cards of format 2. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
Type 
I 
Default 
none 
Shell  Element  Set  Cards.    For  each  shell  element  SID  in  the  intersection  input  one 
field.  Include as many cards as necessary.  This input ends at the next keyword (“*”) 
card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID1 
SSID2 
SSID3 
SSID4 
SSID5 
SSID6 
SSID7 
SSID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
SID 
Set ID of new shell set.  All shell sets should have a unique set ID.
SSID[N] 
The Nth shell set ID
*SET_SOLID_{OPTION1}_{OPTION2} 
For OPTION1 the available options are: 
<BLANK> 
GENERATE 
GENERATE_INCREMENT 
GENERAL 
For OPTION2 the available option is: 
COLLECT 
The GENERATE and GENERATE_INCREMENT options will generate block(s) of solid 
element 
IDs  between  a  starting  ID  and  an  ending  ID.    An  arbitrary  number  of  blocks  can  be 
specified to define the solid element set. 
Purpose:  Define a set of solid elements. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
SOLVER 
Type 
I 
A 
Default 
none  MECH 
Remark
Solid  Element  ID  Cards.    This  Card  2  format  applies  to  the  case  of  an  unset 
(<BLANK>)  keyword  option.    Set  one  value  per  solid  element  in  the  set.    Include  as 
many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 2 
Variable 
1 
K1 
Type 
I 
2 
K2 
I 
3 
K3 
I 
4 
K4 
I 
5 
K5 
I 
6 
K6 
I 
7 
K7 
I 
8 
K8 
I 
Solid  Element  ID  Range  Cards.    This  Card  2  format  applies  to  the  GENERATE 
keyword  option.    Set  one  pair  of  BNBEG  and  BNEND  values  per  block  of  solid 
elements.  Include as many cards as needed.  This input ends at the next keyword (“*”) 
card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
B1BEG 
B1END 
B2BEG 
B2END 
B3BEG 
B3END 
B4BEG 
B4END 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Solid  Element  ID  Range  with  Increment  Cards.    This  Card  2  format  applies  to  the 
GENERATE_INCREMENT keyword option.  For each block of solid elements add one 
card to the deck.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BBEG 
BEND 
INCR 
Type 
I 
I
Generalized  Solid  Element  ID  Range  Cards.    This  Card  2  format  applies  to  the 
GENERAL keyword option.  Include as many cards as needed.  This input ends at the 
next keyword (“*”) card.  
  Card 2 
1 
Variable 
OPTION 
Type 
A 
2 
E1 
I 
3 
E2 
I 
4 
E3 
I 
5 
E4 
I 
6 
E5 
I 
7 
E6 
I 
8 
E7 
I 
  VARIABLE   
DESCRIPTION
SID 
Set ID.  All solid sets should have a unique set ID. 
SOLVER 
Name of solver using this set (MECH, CESE, etc.) 
K1 
K2 
⋮ 
K8 
First element ID 
Second element ID 
⋮  
Eighth element ID 
B[N]BEG 
First solid element ID in block N. 
B[N]END 
BBEG 
BEND 
INCR 
Last  solid  element  ID  in  block  N.    All  defined  ID’s  between  and
including B[N]BEG to B[N]END are added to the set.  These sets 
are  generated  after  all  input  is  read  so  that  gaps  in  the  element
numbering  are  not  a  problem.    B[N]BEG  and  B[N]END  may 
simply be limits on the ID’s and not element IDs. 
First solid element ID in block. 
Last solid element ID in block.   
Solid ID increment.  Solid IDs BBEG, BBEG + INCR, BBEG + 2 ×
INCR,  and so on through BEND are added to the set. 
OPTION 
Option for GENERAL.  See table below. 
E1, ..., E7 
Specified  entity.    Each  card  must  have  the  option  specified.    See
table below.
*SET_SOLID 
The  “OPTION”  column  in  the  table  below  enumerates  the  allowed  values  for  the 
“OPTION” variable in Card 2 for the GENERAL option.  Likewise, the variables E1, …, 
E7 refer to the GENERAL option Card 2. 
Each  of  the  following  operations  accept  up  to  7  arguments,  but  they  may  take  fewer.  
Values of “En” left unspecified are ignored. 
OPTION 
DESCRIPTION 
ALL 
All solid elements will be included in the set. 
ELEM 
Elements E1, E2, E3, ...  will be included. 
DELEM 
Elements E1, E2, E3, ...  previously added will be excluded. 
PART 
Elements of parts E1, E2, E3, ...  will be included. 
DPART 
BOX 
DBOX 
SALECPT 
Elements  of  parts  E1,  E2,  E3,  ...    previously  added  will  be
excluded. 
Elements inside boxes E1, E2, E3, ...  will be included.   
Elements  inside  boxes  E1,  E2,  E3,  ...    previously  added  will  be
excluded. 
Elements inside a box in Structured ALE mesh.  E1 here is the S-
ALE  mesh  ID  (MSHID).    E2,  E3,  E4,  E5,  E6,  E7  correspond  to 
XMIN,  XMAX,  YMIN,  YMAX,  ZMIN,  ZMAX.    They  are  the
minimum  and  the  maximum  nodal  indices  along  each  direction 
in S-ALE mesh.  This option is only to be used for Structured ALE
mesh  and  should  not  be  used  in  a  mixed  manner  with  other 
“_GENERAL” options.    
refer 
Please 
*ALE_STRUCTURED_MESH_CONTROL_-
POINTS and  *ALE_STRUCTURED_MESH_CONTROL for more 
details.   
to
SALEFAC 
*SET 
DESCRIPTION 
Elements  on  the  face  of  Structured  ALE  mesh.    E1  here  is  the  S-
ALE mesh ID (MSHID).  E2, E3, E4, E5, E6, E7 correspond to -X, 
+X,  -Y,  +Y,  -Z,  +Z  faces.    Assigning  1  to  these  6  values  would
include  all  the  boundary  elements  at  these  faces  in  the  segment
set.  This option is only to be used for Structured ALE mesh and
should not be used in a mixed manner with other “_GENERAL” 
options. 
refer 
*ALE_STRUCTURED_MESH_CONTROL_-
Please 
POINTS and  *ALE_STRUCTURED_MESH_CONTROL for more 
details.   
to 
Remarks: 
1.  This  field  is  used  by  a  non-mechanics  solver  to  create  a  set  defined  on  that 
solver’s mesh.  By default, the set refers to the mechanics mesh.
Purpose:  Define a solid set by combining solid sets. 
*SET_SOLID_ADD 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
SOLVER 
Type 
I 
A 
Default 
none  MECH 
Remark 
1 
Node  Set  Cards.    Each  card  can  be  used  to  specify  up  to  8  solid  set  IDs.    Include  as 
many cards as necessary.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID1 
SSID2 
SSID3 
SSID4 
SSID5 
SSID6 
SSID7 
SSID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
SID 
Set ID of new solid set.  All solid sets should have a unique set ID.
SOLVER 
Name of solver using this set (MECH, CESE, etc.) 
SSID[N] 
The Nth solid set ID. 
Remarks: 
1.  This  field  is  used  by  a  non-mechanics  solver  to  create  a  set  defined  on  that 
solver’s mesh.  By default, the set refers to the mechanics mesh.
*SET 
Purpose:  Define a solid set as the intersection, ∩, of a series of solid sets.  The new solid 
set, SID, contains all common elements of all solid sets SSIDn.   
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
SOLVER 
Type 
I 
A 
Default 
none  MECH 
Remark 
1 
Solid  Element  Set  Cards.    For  each  solid  element  SID  in  the  intersection  input  one 
field.  Include as many cards as necessary.  This input ends at the next keyword (“*”) 
card. 
Card 2… 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID1 
SSID2 
SSID3 
SSID4 
SSID5 
SSID6 
SSID7 
SSID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
SID 
Set ID of new solid set.  All solid sets should have a unique set ID.
SOLVER 
Name of solver using this set (MECH, CESE, etc.) 
SSIDN 
The Nth solid set ID on card2 
Remarks: 
1.  This  field  is  used  by  a  non-mechanics  solver  to  create  a  set  defined  on  that 
solver’s mesh.  By default, the set refers to the mechanics mesh.
*SET_TSHELL_{OPTION1}_{OPTION2} 
For OPTION1 the available options are: 
<BLANK> 
GENERATE 
GENERAL 
For OPTION2 the available option is: 
COLLECT 
The  option  GENERATE  will  generate  a  block  of  thick  shell  element  ID’s  between  a 
starting ID and an ending ID.  An arbitrary number of blocks can be specified to define 
the set. 
Purpose:  Define a set of thick shell elements. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
Type 
I 
Default 
none 
Thick  Shell  Element  ID  Cards.    This  Card  2  format  applies  to  the  case  of  an  unset 
(<BLANK>) keyword option.  Set one value per thick shell element in the set.  Include 
as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 2 
Variable 
1 
K1 
Type 
I 
2 
K2 
I 
3 
K3 
I 
4 
K4 
I 
5 
K5 
I 
6 
K6 
I 
7 
K7 
I 
8 
K8
Thick Shell Element ID Range Cards.  This Card 2 format applies to the GENERATE 
keyword  option.    Set  one  pair  of  BNBEG  and  BNEND  values  per  block  of  thick  shell 
elements.  Include as many cards as needed.  This input ends at the next keyword (“*”) 
card. 
Card 2… 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
B1BEG 
B1END 
B2BEG 
B2END 
B3BEG 
B3END 
B4BEG 
B4END 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Generalized Thick Shell Element ID Range Cards.  This Card 2 format applies to the 
GENERAL keyword option.  Include as many cards as needed.  This input ends at the 
next keyword (“*”) card.  
Card 2… 
1 
Variable 
OPTION 
Type 
A 
2 
E1 
I 
3 
E2 
I 
4 
E3 
I 
5 
E4 
I 
6 
E5 
I 
7 
E6 
I 
8 
E7 
I 
  VARIABLE   
DESCRIPTION
SID 
Set ID.  All tshell sets should have a unique set ID. 
K1 
K2 
⋮ 
K8 
First thick shell element ID 
Second thick shell element ID 
⋮  
Eighth thick shell element ID 
B[N]BEG 
First thick shell element ID in block N. 
B[N]END 
Last thick shell element ID in block N.  All defined ID’s between
and including B[N]BEG to B[N]END are added to the set.  These 
sets  are  generated  after  all  input  is  read  so  that  gaps  in  the
element  numbering  are  not  a  problem.    B[N]BEG  and  B[N]END 
may simply be limits on the ID’s and not element IDs. 
OPTION 
Option for GENERAL.  See table below.
E1, ..., E7 
*SET_TSHELL 
DESCRIPTION
Specified  entity.    Each  card  must  have  the  option  specified.    See
table below. 
The General Option: 
The  “OPTION”  column  in  the  table  below  enumerates  the  allowed  values  for  the 
“OPTION” variable in Card 2 for the GENERAL option.  Likewise, the variables E1, …, 
E7 refer to the GENERAL option Card 2. 
Each  of  the  following  operations  accept  up  to  7  arguments,  but  they  may  take  fewer.  
Values of “En” left unspecified are ignored. 
OPTION 
ALL 
ELEM 
DESCRIPTION 
All thick shell elements will be included in the set. 
Elements E1, E2, E3, ...  will be included. 
DELEM 
Elements E1, E2, E3, ...  previously added will be excluded. 
PART 
Elements of parts E1, E2, E3, ...  will be included. 
DPART 
BOX 
DBOX 
Elements  of  parts  E1,  E2,  E3,  ...    previously  added  will  be
excluded. 
Elements  inside  boxes  E1,  E2,  E3,  ...    will  be  included.     
Elements  inside  boxes  E1,  E2,  E3,  ...    previously  added  will  be
excluded.
The keyword *TERMINATION provides an alternative way of stopping the calculation 
before the termination time is reached.  The termination time is specified on the *CON-
TROL_TERMINATION  input  and  will  terminate  the  calculation  whether  or  not  the 
options  available  in  this  section  are  active.    Different  types  of  termination  may  be 
defined:
*TERMINATION_BODY 
Purpose:    Terminate  calculation  based  on  rigid  body  displacements.    For  *TERMINA-
TION_BODY the analysis terminates when the center of mass displacement of the rigid 
body  specified  reaches  either  the  maximum  or  minimum  value  (stops  1,  2 or  3)  or the 
displacement  magnitude  of  the  center  of  mass  is  exceeded  (stop  4).    If  more  than  one 
condition  is  input,  the  analysis  stops  when  any  of  the  conditions  is  satisfied.  
Termination  by  other  means  than  *TERMINATION  input  is  controlled  by  the  *CON-
TROL_TERMINATION  control  card.    Note  that  this  type  of  termination  is  not  active 
during dynamic relaxation. 
Part Cards.  Add one card for each part having termination criterion.  Include as many 
cards as necessary.  This input terminates at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
STOP 
MAXC 
MINC 
Type 
I 
I 
Default 
none 
none 
F 
- 
F 
- 
  VARIABLE   
DESCRIPTION
PID 
STOP 
Part ID of rigid body, see *PART_OPTION. 
Stop criterion: 
EQ.1: global x direction, 
EQ.2: global y direction, 
EQ.3: global z direction, 
EQ.4: stop if displacement magnitude is exceeded. 
MAXC 
Maximum (most positive) displacement, options 1, 2, 3 and 4: 
EQ.0.0: MAXC set to 1.0e21. 
MINC 
Minimum (most negative) displacement, options 1, 2 and 3 above
only: 
EQ.0.0: MINC set to -1.0e21.
*TERMINATION 
Purpose:  The analysis terminates when the magnitude of the contact interface resultant 
force is zero.  If more than one contact condition is input, the analysis stops when any of 
the conditions is satisfied.  Termination by other means than *TERMINATION input is 
controlled  by  the  *CONTROL_TERMINATION  control  card.    Note  that  this  type  of 
termination  is  not  active  during  dynamic  relaxation  and  does  not  apply  to  2D  contact 
types. 
Contact  ID  Cards.    Add  one  card  for  contact  ID  having  a  termination  criterion. 
Include  as  many  cards  as  necessary.    This  input  terminates  at  the  next  keyword  (“*”) 
card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CID 
ACTIM 
DUR 
THRES 
DOF 
Type 
I 
F 
Default 
none 
none 
F 
- 
F 
0.0 
I 
0 
  VARIABLE   
CID 
DESCRIPTION
Contact  ID.    The  contact  ID  is  defined  by  the  ordering  of  the
contact input unless the TITLE option which allows the CID to be
defined is used in the *CONTACT section. 
ACTIM 
Activation time. 
DUR 
THRES 
DOF 
Time  duration  of  null  resultant  force  prior  to  termination.    This 
time  is  tracked  only  after  the  activation  time  is  reached  and  the
contact resultant forces are zero. 
EQ.0.0: Immediate termination after null force is detected. 
Any  measured  force  magnitude  below  or  equal  to  this  specified
threshold is taken as a null force.  Default = 0.0 
Option  to  consider  only  the  force  magnitude  in  the  x,  y,  or  z
global directions corresponding to DOF = 1,2, and 3, respectively.
*TERMINATION_CURVE 
Purpose:    Terminate  the  calculation  when  the  load  curve  value  returns  to  zero.    This 
termination  can  be  used  with  the  contact  option  *CONTACT_AUTO_MOVE.      In  this 
latter  option,  the  load  curve  is  modified  to  account  for  the  movement  of  the  master 
surface. 
Load  Curve  Card.    For  each  load  curve  used  as  a  termination  criterion  add  a  card. 
Include as many cards as necessary.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
ATIME 
Type 
I 
F 
Default 
none 
Remark 
1 
- 
  VARIABLE   
DESCRIPTION
LCID 
Load curve ID governing termination. 
ATIME 
Activation  time.    After  this  time  the  load  curve  is  checked.    If
zero, see remark 1 below. 
Remarks: 
1. 
If  ATIME = 0.0,  termination  will  occur  after  the  load  curve  value  becomes 
nonzero and then returns to zero.
*TERMINATION_DELETED_SHELLS_{OPTION} 
Available options include: 
<BLANK> 
SET 
Purpose:    Terminate  the  calculation  when  the  number  of  deleted  shells  for  a  specified 
part ID exceeds the value defined here.  This input has no effect for a part ID that is left 
undefined.    Generally,  this  option  should  be  used  with  the  NFAIL1  and  NFAIL4 
parameters that are defined in the *CONTROL_SHELL control information. 
When using the SET option, termination will occur when NDS elements are deleted in 
any one of the parts in the part set PSID.  
Part (set) Cards.  Include one card for each part having a termination criterion based 
on  shell  deletion.    Include  as  many  cards  as  necessary.    This  input  ends  at  the  next 
keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID/PSID 
NDS 
Type 
I 
I 
Default 
none 
none 
  VARIABLE   
DESCRIPTION
PID / PSID 
Part ID or if option SET is active, part set ID. 
NDS 
Number  of  elements  that  must  be  deleted  for  the  specified  part
ID’s, before an error termination occurs.
*TERMINATION_DELETED_SOLIDS_{OPTION} 
Available options include: 
<BLANK> 
SET 
Purpose:    Terminate  the  calculation  when  the  number  of  deleted solids  for  a  specified 
part ID exceeds the value defined here.  This input has no effect for a part ID that is left 
undefined. 
When using the SET option, termination will occur when NDS elements are deleted in 
any one of the parts in the part set PSID.   
Part (set) Cards.  Include one card for each part having a termination criterion based 
on solid element deletion.  Include as many cards as necessary.  This input ends at the 
next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID/PSID 
NDS 
Type 
I 
Default 
none 
I 
1 
  VARIABLE   
DESCRIPTION
PID/PSID 
Part ID or if option SET is active, part set ID. 
NDS 
Number  of  elements  that  must  be  deleted  for  the  specified  part
ID’s, before an error termination occurs.
*TERMINATION 
Purpose:    Terminate  calculation  based  on  nodal  point  coordinates.    The  analysis 
terminates for *TERMINATION_NODE when the current position of the node specified 
reaches either the maximum or minimum value (stops 1, 2 or 3), or picks up force from 
any  contact  surface  (stops  4).    Termination  by  other  means  than  *TERMINATION  is 
controlled  by  the  *CONTROL_TERMINATION  control  card.    Note  that  this  type  of 
termination is not active during dynamic relaxation. 
Node Cards.  Include one card for each node having a termination criterion.  Include as 
many cards as desired.  This input terminates at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID 
STOP 
MAXC 
MINC 
Type 
I 
I 
Default 
none 
none 
F 
- 
F 
- 
  VARIABLE   
DESCRIPTION
NID 
STOP 
MAXC 
MINC 
Node ID, see *NODE_OPTION. 
Stop criterion: 
EQ.1: global x direction, 
EQ.2: global y direction, 
EQ.3: global z direction, 
EQ.4: stop if node touches contact surface. 
Maximum  (most  positive)  coordinate  (options  1,  2  and  3)  above
only. 
Minimum  (most  negative)  coordinate  (options  1,  2  and  3)  above
only.
*TERMINATION_SENSOR 
Purpose:  Terminates the calculation when the switch condition defined in *SENSOR_-
SWITCH is met. 
Switch ID Cards.  Include one card for each switch controlling termination.  Include as 
many cards as desired.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SWID 
Type 
I 
Default 
none 
  VARIABLE   
SWID 
Remarks: 
DESCRIPTION
ID  of  *SENSOR_SWITCH  which  will  terminate  the  calculation
when  its  condition  is  met.    Only  one  *TERMINATION_SENSOR 
is  allowed.    If  more  than  one  *TERMINATION_SENSOR  is 
defined; only the last one is effective.   
An example allowing more than one sensor_switch to terminate calculation: 
*SENSOR_DEFINE_ELEMENT 
$ Axial force of beam element 1 
44,BEAM,1,AXIAL,FORCE 
*SENSOR_DEFINE_ELEMENT 
$ Axial force of beam element 2 
55,BEAM,21,AXIAL,FORCE 
*SENSOR_SWITCH 
$a switch condition is  met when the axial force of beam-1 >5.0 
11,SENSOR,44,GT,5. 
*SENSOR_SWITCH 
$a switch condition is  met when the axial force of beam-2 >10.0 
22,SENSOR,55,GT,10. 
*SENSOR_SWITCH 
$ a switch condition is  met when time >50. 
33,TIME, , 50 
*SENSOR_SWITCH_CALC-LOGIC 
$ a switch condition is met if both conditions 
$ of switch-11 and switch-33 are met, I.e.,  
$ axial force of beam-1>5.0 and time>50 
44,11,33 
*SENSOR_SWITCH_CALC-LOGIC 
$ a switch condition is met if both conditions 
$ of switch-22 and switch-33 are met, I.e.,
$ axial force of beam-2>10.0 and time>50 
55,33,22 
*SENSOR_SWITCH_CALC-LOGIC 
$ a switch condition is met if the conditions 
$ of switch-44 or switch-55 is met, I.e.,  
$ axial force of beam-1>5.0 and time>50 or 
$ axial force of beam-2>10.0 and time>50 
66,44,-55 
*TERMINATION_SENSOR 
$ job will be terminated when the switch condition of switch-66 is met, I.e., 
$ axial force of beam-1>5.0 and time>50 or 
$ axial force of beam-2>10.0 and time>50 
66
*TITLE 
Purpose:  Define job title. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
TITLE 
C 
LS-DYNA USER INPUT 
  VARIABLE   
DESCRIPTION
TITLE 
Heading to appear on output and in output files.
*USER_INTERFACE_OPTION 
Available options include: 
CONTROL 
FRICTION 
FORCES 
CONDUCTIVITY 
Purpose:    Define  user  defined  input  and  allocate  storage  for  user  defined  subroutines 
for  the  contact  algorithms.    See  also  *CONTROL_CONTACT.    The  CONTROL  option 
above allows the user to take information from the contact interface for further action, 
e.g., stopping the analysis.  A sample user subroutine is provided in Appendix F. 
or 
The  FRICTION  option  may  be  used  to  modify  the  Coulomb  friction  coefficients  in 
contact  types  3,  5,  or  10  (*CONTACT_SURFACE_TO_SURFACE,  *CONTACT_-
NODES_TO_SURFACE, 
*CONTACT_ONE_WAY_SURFACE_TO_SURFACE) 
according  to  contact  information  or  to  use  a  friction  coefficient  database.    A  sample 
user-defined friction subroutine is provided in Appendix G.   For the subroutine to be 
called,  the  static  friction  coefficient  FS  on  Card  2  of  *CONTACT  must  be  any  nonzero 
value, and shell thickness offsets must be invoked in the contact by setting SHLTHK to 
1 or 2 using *CONTROL_CONTACT or Opt.  Card B in *CONTACT.  The array length 
USRFRC in *CONTROL_CONTACT should be set to a value no less than the sum of the 
number of history variables NOC and the number of user-defined input parameters in 
*USER_INTERFACE_FRICTION. 
The  CONDUCTIVITY  option  is  used  to  define  heat  transfer  contact  conductance 
properties for thermal contacts. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IFID 
NOC 
NOCI 
NHSV 
Type 
I 
I 
I 
I 
Default 
none 
none 
none
Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
UC1 
UC2 
UC3 
UC4 
UC5 
UC6 
UC7 
UC8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
IFID 
NOC 
NOCI 
NHSV 
UC1 
UC2 
⋮ 
Interface number 
Number  of  history  variables  for  interface.    The  number  should
not exceed the length of the array defined on *CONTROL_CON-
TACT.  See Remarks. 
Initialize  the  first  NOCI  history  variables  in  the  input.    NOCI
must be smaller or equal to NOC. 
Number  of  history  variables  per  interface  node  (only  for  friction
and conductivity interface). 
First user defined input parameter. 
Second user defined input parameter. 
⋮  
UC[N] 
Last user defined input parameter, where N = NOCI. 
The FORCES option is used to collect contact nodal forces from specified contact ID list 
for user subroutines. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NCONT 
Type 
I 
Default 
none
Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CID1 
CID2 
CID3 
CID4 
CID5 
CID6 
CID7 
CID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
IFID 
Interface number 
NCONT 
Number of contact ID.  If NCONT LE.  0, all contacts will be used.
CID1 
CID2 
⋮ 
First contact user ID. 
Second contact user ID. 
⋮  
CID[N] 
Last contact user ID, where N = NCONT. 
Remarks: 
The (NOC) interface variables (of which NOCI are initialized) are passed as arguments 
to the user defined subroutine.  See Appendix G for the full list of arguments passed to 
the subroutine. 
This  keyword  is  not  supported  by  segment  based  contact  which  is  invoked  by  setting 
SOFT = 2 on optional card A of the *CONTACT card.
*USER_LOADING 
Purpose:    Provide  a  means  of  applying  pressure  and  force  boundary  conditions.    The 
keyword *USER_LOADING activates this option.  Input here is optional with the input 
being read until the next “*” keyword appears.  The data read here is to be stored in a 
common  block  provided  in  the  user  subroutine,  LOADUD.    This  data  is  stored  and 
retrieved from the restart files. 
Parameter Cards.  Add one card for each input parameter.  Include as many cards as 
needed.  This input ends at the next keyword (“*”) card. 
Card 1… 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PARM1 
PARM2 
PARM3 
PARM4 
PARM5 
PARM6 
PARM7 
PARM8 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
PARM[N] 
This is the Nth user input parameter.
*USER 
Purpose:  Provides a means to apply user-defined loading to a set of nodes or segments.  
Loading  could  be  nodal  force,  body  force,  temperature  distribution,  and  pressure  on 
segment or beam. 
Set Cards.  Add a card for each set to which a load is applied.  Include as many cards 
as necessary.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
LTYPE 
LCID 
CID 
SF1 
SF2 
SF3 
IDULS 
Type 
I 
A 
I 
I 
F 
F 
F 
I 
Default 
none 
none 
none 
global 
none 
none 
none 
Seq.  #
  VARIABLE   
SID 
DESCRIPTION
ID  of  the  set  to  which  user-defined  loading  will  be  applied.    Set 
type depends on the type of loading, see LTYPE. 
LTYPE 
Loading type: 
EQ.“FORCEN”:  Force  a  will  be  applied  to  node  set  SID.    The
load is to be given in units of force. 
EQ.“BODYFN”:  Body force density will be applied to node set
SID.    The  load  is  to  be  given  in  units  of  force
per volume. 
EQ.“TEMPTN”:  Temperature will be assigned to node set SID.
This  option  cannot  be  coexist  with  *LOAD_-
THERMAL_VARIABLE.    In  other  word,  users 
can  only  use  either  this  option  or  *LOAD_-
THERMAL_VARIABLE to specify temperature 
distribution, not both of them, 
EQ.“PRESSS”:  Pressure  will  be  applied  to  segment  set  SID.
The load is to be given in units of force per ar-
ea. 
EQ.“PRESSB”:  Pressure  in  units  of  force  per  length  will  be
applied to beam set SID.
LCID 
CID 
*USER_LOADING_SET 
DESCRIPTION
Load curve, a function of time.  Its current value, crv, is passed to 
user subroutine LOADSETUD. 
Optional  coordinate  system  along  which  scale  factors  SFi  is 
defined.  Global system is the default system. 
SF[i] 
Scale factor of loading magnitude, when LTYPE 
LTYPE.EQ.“FORCEN”:  SFi  is  the  factor  along  𝑖th  direction  of 
CID.  For example, set SF1 = 1.  and the 
others  to  zero  if  the  load  is  to  be  ap-
plied  in  the  positive  𝑥-direction.    This 
applies  whether  the  global  or  a  local 
coordinate system is used. 
LTYPE.EQ.“BODYFN”:  See “EQ.FORCEN” 
LTYPE.EQ.“PRESSS”:  SF1 is used as the scale factor, SF2 and 
SF3 are ignored, 
LTYPE.EQ.“PRESSB”:  Scale factor along 𝑟, 𝑠, 𝑡 axis of beam. 
Each  USER_LOADING_SET  can  be  assigned  a  unique  ID,  which 
is  passed  to  user  subroutine  LOADSETUD  and  allows  multiple 
loading  definitions  by  using  a  single  user  subroutine,  LOADSE-
TUD.    If  no  value  is  input,  LS-DYNA  will  assign  a  sequence 
number  to  each  USER_LOADING_SET  based  on  its  definition 
sequence. 
IDULS 
Remarks: 
*USER_LOADING_SET activates the loading defined in user subroutine LOADSETUD, 
part  of  dyn21.F.    When  both  *USER_LOADING_SET  and  *USER_LOADING  are 
defined,  *USER_LOADING  is  only  used  to  define  user-defined  parameters,  PARMn; 
not  to  activate  user  subroutine  LOADUD.    Therefore  only  loading  defined  in 
LOADSETUD will be applied.   
More  than  one  loading  definitions  can  be  defined  and  assigned  a  unique  ID,  that 
enables  multiple  loading  to  be  taken  care  of  by  a  single  subroutine,  LOADSETUD,  as 
shown below: 
subroutine loadsetud(time,lft,llt,crv,iduls,parm) 
c 
c     Input (not modifiable) 
c       x   : coordinate of node or element center 
c       d   : displacement of node or element center 
c       v   : velocity of node or element center
c       temp: temperature of node or element center 
c       crv : value of LCID at current time 
c     isuls : id of user_loading_set 
c     parm: parameters defined in *USER_LOADING 
c     Output (defined by user) 
c       udl : user-defined load value 
      include 'nlqparm' 
C_TASKCOMMON (aux8loc) 
      common/aux8loc/ 
     & x1(nlq),x2(nlq),x3(nlq),v1(nlq),v2(nlq),v3(nlq), 
     & d1(nlq),d2(nlq),d3(nlq),temp(nlq),udl(nlq),tmp(nlq,12) 
c 
c    sample code 
c    if (iduls.eq.100) then  
c      do i=lft,llt 
c       your code here 
c        udl(i)=.......... 
c      enddo 
c    elseif (iduls.eq.200) then 
c      do i=lft,llt 
c        udl(i)=.......... 
c      enddo 
c    endif 
      return 
      end
Restart Input Data 
Restart Input Data 
In  general  three  categories  of  restart  actions  are  possible  with  LS-DYNA  and  are 
outlined in the following discussion: 
1.  A  simple  restart  occurs  when  LS-DYNA  was  interactively  stopped  before 
reaching  the  termination  time.    Then,  by  specifying  the  R=rtf  command  line 
option on the execution line, LS-DYNA restarts the calculation from the termi-
nation  point.      The  calculation  will  pick  up  at  the  specified  termination  time.  
see INTRODUCTION, Execution Syntax.  No additional input deck is required. 
2.  For  small  modifications  of  the  restart  run  LS-DYNA  offer  a  “small  restart” 
capability which can 
a)  reset termination time, 
b)  reset output printing interval, 
c)  reset output plotting interval, 
d)  delete contact surfaces, 
e)  delete elements and parts, 
f)  switch deformable bodies to rigid, 
g)  switch rigid bodies to deformable, 
h)  change damping options. 
All  modifications  to  the  problem  made  with  the  restart  input  deck  will  be  re-
flected  in  subsequent  restart  dumps.    All  the  members  of  the  file  families  are 
consecutively numbered beginning from the last member prior to termination. 
For a small restart run a small input deck replaces the standard input deck on the 
execution line which must have at least the following command line arguments: 
LS-DYNA I=restartinput R=D3DUMPnn 
where D3DUMPnn  (or whatever name is chosen for the family member) is the 
nth restart file from the last run where the data is taken.  LS-DYNA automati-
cally  detects  that  a  small  input  deck  is  used  since  the  I=restartinput  file  may 
contain only the restart keywords (excluding *STRESS_INITIALIZATION): 
*CHANGE_OPTION
*CONTROL_SHELL 
*CONTROL_TERMINATION 
*CONTROL_TIMESTEP 
*DAMPING_GLOBAL 
*DATABASE_OPTION 
*DATABASE_BINARY_OPTION 
*DELETE_OPTION 
*INTERFACE_SPRINGBACK_LSDYNA 
*RIGID_DEFORMABLE_OPTION 
*STRESS_INITIALIZATION_{OPTION} 
*TERMINATION_OPTION 
*TITLE 
*KEYWORD 
*CONTROL_CPU 
*DEFINE_OPTION 
*SET_OPTION 
The user has to take care that nonphysical modifications to the input deck are 
avoided; otherwise, complete nonsense may be the result. 
3. 
If many modifications are desired a full restart may be the appropriate choice.  A 
full restart is selected by including a full model along with a *STRESS_INITIAL-
IZATION keyword card and possibly other restart cards.  As mentioned in the 
Restart  Analysis  subsection  of  the  Introduction  portion  of  the  manual,  either  all 
parts or some subset of parts can be made for the stress initialization. 
Remarks: 
a)  In a full restart, only those nodes and elements defined in the full restart 
deck will be present in the analysis after the full restart is initiated.  But as 
a  convenience,  any  of  those  nodes  or  elements  can  be  deleted  using  the 
*DELETE command.
Restart Input Data 
b)  In a small restart, velocities of nodes come from the dump file by default 
but those velocities can be changed using *CHANGE_VELOCITY_....   
c)  In a full restart, velocities of pre-existing nodes come from the dump file 
by default but those velocities can be changed using *CHANGE_VELOCI-
TY_....    To  set  the  starting  velocities  for  new  nodes  in  a  full  restart,  use 
*INITIAL_VELOCITY_.... 
d)  Pre-existing contacts, in general, carry forward seamlessly using data from 
the  d3dump  (or  d3full  if  MPP)  database.    It  is  important  that  the  contact 
ID(s) in the full restart input deck match the contact ID(s) in the original 
input deck if the intent is for the contacts to be initialized using data from 
the d3dump/d3full database.  EXCEPTION:  In the special case of MPP, a 
*CONTACT_AUTOMATIC_GENERAL  contact  in  the  full  restart  input 
deck  is  treated  as  a  brand  new  contact  and  is  not  initialized  using  data 
from d3full. 
e)  Only sets utilizing element IDs and node IDs are permitted in a small re-
start  deck;  part  IDs  are  not  recognized.    Sets  referenced  by  other  com-
mands in a small restart deck must be defined in the small restart deck.
*CHANGE_OPTION 
Purpose:  Change solution options. 
Available options include: 
BOUNDARY_CONDITION 
CONTACT_SMALL_PENETRATION 
CURVE_DEFINITION 
OUTPUT 
RIGIDWALL_GEOMETRIC 
RIGIDWALL_PLANAR 
RIGID_BODY_CONSTRAINT 
RIGID_BODY_INERTIA 
RIGID_BODY_STOPPER 
STATUS_REPORT_FREQUENCY 
THERMAL_PARAMETERS 
VELOCITY 
VELOCITY_GENERATION 
VELOCITY_NODE 
VELOCITY_RIGID_BODY 
VELOCITY_ZERO 
Boundary  Condition  Cards.    This  card  1  format  is  for  the  BOUNDARY_CONDITION 
keyword  option.    Add  one  card  for  each  boundary  condition.    This  card  imposes 
additional boundary conditions.  It does not remove previously imposed conditions (for 
example,  this  option  will  not  free  a  fixed  node).    This  input  ends  at  the  next keyword 
(“*”) card.
Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID 
BCC 
Type 
I 
I 
  VARIABLE   
DESCRIPTION
NID 
BCC 
Nodal point ID, see also *NODE. 
New translational boundary condition code: 
EQ.1: constrained 𝑥 displacement, 
EQ.2: constrained 𝑦 displacement, 
EQ.3: constrained 𝑧 displacement, 
EQ.4: constrained 𝑥 and 𝑦 displacements, 
EQ.5: constrained 𝑦 and 𝑧 displacements, 
EQ.6: constrained 𝑧 and 𝑥 displacements, 
EQ.7: constrained 𝑥, 𝑦, and 𝑧 displacements. 
Small  Penetration  Check  Cards.    This  Card  1  format  is  for  the  CONTACT_SMALL_
PENETRATION keyword option.  Set one value for each contact surface ID where the 
small penetration check is to be turned on.   The input terminates  at the next keyword 
(“*”) card.  See the PENCHK variable in *CONTACT. 
  Card 1 
1 
Variable 
ID1 
2 
ID2 
3 
ID3 
4 
ID4 
5 
ID5 
6 
ID6 
7 
ID7 
8 
ID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
IDn 
Contact ID for surface number n. 
Load Curve Redefinition Cards.  This Card 1 format is for the CURVE_DEFINITION 
keyword option.  The new load curve must contain the same number of points as the curve it 
replaces.  The curve should be defined according to the DEFINE_CURVE section of the 
manual.  This input terminates when the next “*” card is encountered.  Offsets and scale 
factors are ignored.
Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
Type 
I 
  VARIABLE   
DESCRIPTION
LCID 
Load curve ID 
ASCII Output Overwrite Card.  This format applies to the OUTPUT keyword option. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IASCII 
Type 
I 
  VARIABLE   
IASCII 
DESCRIPTION
Flag  to  control  manner  of  outputing  ASCII  data  requested  by
*DATABASE_OPTION commands in a full restart deck: 
EQ.0: Full restart overwrites existing ASCII output (default), 
EQ.1: Full restart appends to existing ASCII output. 
Rigidwall  modification. 
  The  format  for  the  RIGIDWALL_GEOMETRIC  and 
RIGIDWALL_PLANAR cards is identical to the original cards ,  however  there  are  restrictions  on  the  entries 
that may be changed: only those entries that define the size and orientation of the rigid 
walls may be changed, but not any of the others (e.g., the type). 
Rigid  Body  Constraint  Modification  Cards.    This  format  for  Card  1  applies  to  the 
RIGID_BODY_CONSTRAINT keyword option.  This option can change translation and 
rotational  boundary  condition  on  a  rigid  body.    This  input  ends  at  the  next  keyword 
(“*”) card.  See CONSTRAINTED_RIGID_BODIES.
1 
Variable 
PID 
Type 
I 
2 
TC 
I 
3 
RC 
I 
*RESTART INPUT DATA 
4 
5 
6 
7 
8 
  VARIABLE   
DESCRIPTION
PID 
TC 
Part ID, see *PART. 
Translational constraint: 
EQ.0: no constraints, 
EQ.1: constrained 𝑥 displacement, 
EQ.2: constrained 𝑦 displacement, 
EQ.3: constrained 𝑧 displacement, 
EQ.4: constrained 𝑥 and 𝑦 displacements, 
EQ.5: constrained 𝑦 and 𝑧 displacements, 
EQ.6: constrained 𝑧 and 𝑥 displacements, 
EQ.7: constrained 𝑥, 𝑦, and 𝑧 displacements. 
RC 
Rotational constraint: 
EQ.0: no constraints, 
EQ.1: constrained 𝑥 rotation, 
EQ.2: constrained 𝑦 rotation, 
EQ.3: constrained 𝑧 rotation, 
EQ.4: constrained 𝑥 and 𝑦 rotations, 
EQ.5: constrained 𝑦 and 𝑧 rotations, 
EQ.6: constrained 𝑧 and 𝑥 rotations, 
EQ.7: constrained 𝑥, 𝑦, and 𝑧 rotations. 
Card  sets  for  RIGID_BODY_INERTIA  keyword  option.    This  option  supports 
changing the mass and inertia properties of a rigid body.  Include as many pairs of the 
following two cards as necessary.  This input ends at the next keyword (“*”) card.  The 
inertia  tensor  is  specified  relative  to  the  coordinate  system  set  in  *MAT_RIGID  at  the 
start  of  the  calculation,  which  is  fixed  in  the  rigid  body  and  tracks  the  rigid  body 
rotation.
Card 1 
Variable 
1 
ID 
2 
PID 
3 
TM 
Type 
I 
I 
F 
4 
5 
6 
7 
8 
  Card 2 
1 
Variable 
IXX 
2 
IXY 
3 
IXZ 
4 
IYY 
5 
IYZ 
6 
IZZ 
7 
8 
Type 
F 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION
ID 
PID 
TM 
IXX 
IXY 
IXZ 
IYY 
IYZ 
IZZ 
ID for this change inertia input. 
Part ID, see *PART. 
Translational mass. 
𝐼𝑥𝑥, 𝑥𝑥 component of inertia tensor. 
𝐼𝑥𝑦  
𝐼𝑥𝑧  
𝐼𝑦𝑦  
𝐼𝑦𝑧  
𝐼𝑧𝑧  
Card  sets  for  the  RIGID_BODY_STOPPERS  keyword  option.    This  option  is  for 
redefining  existing  stoppers.    Include  as  many  pairs  of  cards  as  necessary.    This  input 
terminates  when  the  next  “*”  card  is  encountered.    See  *CONSTRAINED_RIGID_-
BODY_STOPPERS.    Note  that  new  stopper  definitions  cannot  be  introduced  in  this 
section.  Existing stoppers can be modified.
Card 1 
1 
2 
3 
4 
5 
6 
7 
Variable 
PID 
LCMAX 
LCMIN 
PSIDMX 
PSIDMN 
LCVMNX 
DIR 
8 
VID 
I 
0 
3 
I 
0 
4 
I 
0 
5 
I 
I 
I 
0 
required 
0 
6 
7 
8 
Type 
I 
I 
Default 
required 
0 
  Card 2 
1 
2 
Variable 
BIRTH 
DEATH 
Type 
Default 
F 
0 
F 
1028 
  VARIABLE   
DESCRIPTION
PID 
Part ID of master rigid body, see *PART. 
LCMAX 
Load curve ID defining the maximum coordinate as a function of 
time: 
EQ.0: no  limitation  of  the  maximum  displacement.    New
curves  can  be  defined  by  the  *DEFINE_CURVE  within 
the  present  restart  deck.    (Not  applicable  for  small  deck
restart). 
LCMIN 
Load curve ID defining the minimum coordinate as a function of 
time: 
EQ.0: no limitation of the minimum displacement.  New curves
can be defined by the  *DEFINE_CURVE within the pre-
sent restart deck.  (Not applicable for small deck restart).
PSIDMX 
Optional  part  set  ID  of  rigid  bodies  that  are  slaved  in  the
maximum  coordinate  direction  to  the  master  rigid  body.    This
option requires additional input by the *SET_PART definition.
VARIABLE   
PSIDMN 
DESCRIPTION
Optional  part  set  ID  of  rigid  bodies  that  are  slaved  in  the
minimum  coordinate  direction  to  the  master  rigid  body.    This
option requires additional input by the *SET_PART definition. 
LCVMNX 
Load curve ID which defines the maximum absolute value of the
velocity that is allowed within the stopper: 
EQ.0: no limitation of the minimum displacement. 
DIR 
Direction stopper acts in: 
EQ.1: 𝑥-translation, 
EQ.2: 𝑦-translation, 
EQ.3: 𝑧-translation, 
EQ.4: arbitrary, defined by vector VID, 
EQ.5: 𝑥-axis rotation, 
EQ.6: 𝑦-axis rotation, 
EQ.7: 𝑧-axis rotation, 
EQ.8: arbitrary, defined by vector VID. 
VID 
Vector  for  arbitrary  orientation  of  stopper.    The  vector  must  be
defined by a *DEFINE_VECTOR within the present restart deck. 
BIRTH 
Time at which stopper is activated. 
DEATH 
Time at which stopper is deactivated. 
Remarks: 
The  optional  definition  of  part  sets  in  minimum  or  maximum  coordinate  directions 
allows the motion to be controlled in an arbitrary direction. 
D3HSP  Interval  Change  Card.  This  card  format  applies  to  the  STATUS_REPORT_
FREQUENCY keyword option. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IKEDIT 
Type
VARIABLE   
DESCRIPTION
IKEDIT 
Problem status report interval steps in the D3HSP output file: 
EQ.0: interval remains unchanged. 
Card  set  for  the  THERMAL_PARAMETERS  keyword  option.    This  option  is  for 
changing the parameters used by a thermal or coupled structural/thermal analysis.  See  
*CONTROL_THERMAL.  Add the two following cards to the deck (they do not repeat). 
3 
4 
5 
6 
7 
8 
TMIN 
TMAX 
DTEMP 
TSCP 
F 
3 
F 
4 
F 
5 
F 
6 
7 
8 
  Card 1 
Variable 
1 
TS 
Type 
I 
  Card 2 
1 
2 
DT 
F 
2 
Variable 
REFMAX 
TOL 
Type 
I 
F 
  VARIABLE   
DESCRIPTION
TS 
Thermal time step code: 
EQ.0: No change, 
EQ.1: Fixed time step, 
EQ.2: variable time step. 
DT 
Thermal time step on restart: 
EQ.0: No change. 
TMIN 
Minimum thermal time step: 
EQ.0: No change. 
TMAX 
Maximum thermal time step: 
EQ.0: No change.
VARIABLE   
DESCRIPTION
DTEMP 
Maximum temperature change in a thermal time step: 
EQ.0: No change. 
TSCP 
Time step control parameter  (0.0 < TSCP < 1.0 ): 
EQ.0: No change. 
REFMAX 
Maximum number of reformations per thermal time step: 
EQ.0: No change. 
TOL 
Non-linear convergence tolerance: 
EQ.0: No change. 
Node Set Velocity Card Sets.  The formats for Cards 1 and 2 apply to the VELOCITY 
and  VELOCITY_ONLY  keyword  options.    These  options  are  for  setting  velocity  fields 
on  node  sets  at  restart.    For  each  node  set  add  one  pair  of  the  following  cards.    This 
input ends at the next keyword (“*”) card.  Undefined nodes (not listed on a set velocity 
card) will have their nodal velocities reset to zero if a *CHANGE_VELOCITY definition 
is  encountered  in  the  restart  deck.    However,  if  any  of  the  *CHANGE_VELOCITY 
definitions  have  ONLY  appended,  then only  the  specified  nodes  will  have  their  nodal 
velocities modified. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSID 
Type 
I 
Default 
none 
Remark
Variable 
1 
VX 
Type 
F 
Default 
0. 
2 
VY 
F 
0. 
3 
VZ 
F 
0. 
*RESTART INPUT DATA 
4 
5 
6 
7 
8 
VXR 
VYR 
VZR 
F 
0. 
F 
0. 
F 
0. 
  VARIABLE   
DESCRIPTION
NSID 
Nodal set ID containing nodes for initial velocity. 
Velocity in 𝑥-direction. 
Velocity in 𝑦-direction. 
Velocity in 𝑧-direction. 
Rotational velocity about the 𝑥-axis. 
Rotational velocity about the 𝑦-axis. 
Rotational velocity about the 𝑧-axis. 
VX 
VY 
VZ 
VXR 
VYR 
VZR 
Remarks: 
1. 
If a node is initialized on more than one input card set, then the last set input 
will determine its velocity, unless it is specified on a *CHANGE_VELOCITY_-
NODE card. 
2.  Undefined nodes will have their nodal velocities set to zero if a *CHANGE_VE-
LOCITY definition is encountered in the restart deck. 
3. 
If  both  *CHANGE_VELOCITY  and  *CHANGE_VELOCITY_ZERO  cards  are 
defined then all velocities will be reset to zero. 
Velocity  generation  cards.    The  velocity  generation  cards  for  the  VELOCITY_
GENERATION option are identical to the standard velocity generation cards , and all parameters may be changed.
Nodal  Point  Velocity  Cards.    This  format  applies  to  the  VELOCITY_NODE  and 
VELOCITY_NODE_ONLY  keyword  options.    These  option  support  changing  nodal 
velocities.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
Variable 
NID 
Type 
I 
2 
VX 
F 
Default 
none 
0. 
3 
VY 
F 
0. 
4 
VZ 
F 
0. 
5 
6 
7 
8 
VXR 
VYR 
VZR 
F 
0. 
F 
0. 
F 
0. 
  VARIABLE   
DESCRIPTION
NID 
Node ID 
Translational velocity in 𝑥-direction. 
Translational velocity in 𝑦-direction. 
Translational velocity in 𝑧-direction. 
Rotational velocity about the 𝑥-axis. 
Rotational velocity about the 𝑦-axis. 
Rotational velocity about the 𝑧-axis. 
VX 
VY 
VZ 
VXR 
VYR 
VZR 
Remarks: 
1.  Undefined  nodes  (not  listed  on  a  point  velocity  card)  will  have  their  nodal 
velocities reset to zero if a *CHANGE_VELOCITY_NODE definition is encoun-
tered  in  the  restart  deck.    However,  if  any  of  the  *CHANGE_VELOCITY  or 
CHANGE_VELOCITY_NODE  definitions  have_ONLY  appended,  then  only 
the specified nodes will have their nodal velocities modified. 
2. 
3. 
If a node is initialized on more than one input card set, then the last set input 
will determine its velocity, unless it is specified on a *CHANGE_VELOCITY_-
NODE card. 
If  both  *CHANGE_VELOCITY  and  *CHANGE_VELOCITY_ZERO  cards  are 
defined then all velocities will be reset to zero.
Rigid  Body  Velocity  Cards.    This  Card  1  format  applies  to  the  VELOCITY_RIGID_
BODY  keyword  option.    This  option  allows  for  setting  the  velocity  components  of  a 
rigid body at restart.  Include as many of these cards as desired.  This input ends at the 
next keyword (“*”) card. 
  Card 1 
1 
Variable 
PID 
Type 
I 
2 
VX 
F 
Default 
none 
0. 
3 
VY 
F 
0. 
4 
VZ 
F 
0. 
5 
6 
7 
8 
VXR 
VYR 
VZR 
F 
0. 
F 
0. 
F 
0. 
  VARIABLE   
DESCRIPTION
Part ID of rigid body. 
Translational velocity in 𝑥-direction. 
Translational velocity in 𝑦-direction. 
Translational velocity in 𝑧-direction. 
Rotational velocity about the 𝑥-axis. 
Rotational velocity about the 𝑦-axis. 
Rotational velocity about the 𝑧-axis. 
PID 
VX 
VY 
VZ 
VXR 
VYR 
VZR 
Remarks: 
1.  Rotational velocities are defined about the center of mass of the rigid body. 
2.  Rigid bodies not defined in this section will not have their velocities modified. 
Restarting  the  Model  at  Rest.    The  VELOCITY_ZERO  option  resets  the  velocities  to 
zero at the start of the restart.  There are no data cards associated with *CHANGE_VE-
LOCITY_ZERO.
*CONTROL_DYNAMIC_RELAXATION 
Purpose:  Define controls for dynamic relaxation. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NRCYCK 
DRTOL 
DRFCTR  DRTERM 
TSSFDR 
IRELAL 
EDTTL 
IDRFLG 
Type 
I 
F 
F 
F 
F 
Default 
250 
0.001 
0.995 
∞ 
TSSFAC 
Remarks 
1 
1 
1 
1 
1 
I 
0 
F 
0.0 
I 
0 
1 
  VARIABLE   
NRCYCK 
DESCRIPTION
Number  of  iterations  between  convergence  checks,  for  dynamic 
relaxation option (default = 250). 
DRTOL 
Convergence 
(default = 0.001). 
tolerance 
for  dynamic 
relaxation 
option
DRFCTR 
Dynamic relaxation factor (default = .995). 
DRTERM 
TSSFDR 
IRELAL 
EDTTL 
Optional  termination  time  for  dynamic  relaxation.    Termination
occurs  at  this  time  or  when  convergence  is  attained  (de-
fault = infinity). 
Scale factor for computed time step during dynamic relaxation.  If
zero, the value is set to TSSFAC defined on *CONTROL_TERMI-
NATION.  After converging, the scale factor is reset to TSSFAC. 
Automatic  control  for  dynamic  relaxation  option  based  on
algorithm of Papadrakakis [1981]. 
Convergence 
relaxation. 
tolerance  on  automatic  control  of  dynamic
IDRFLG 
Dynamic relaxation flag for stress initialization: 
EQ.0: not active, 
EQ.1: dynamic relaxation is activated.
Remarks: 
1. 
2. 
If  a  dynamic  relaxation  relaxation  analysis  is  being  restarted  at  a  point  before 
convergence  was  obtained,  then  NRCYCK,  DRTOL,  DRFCTR,  DRTERM  and 
TSSFDR will default to their previous values, and IDRFLG will be set to 1. 
If  dynamic  relaxation  is  activated  after  a  restart  from  a  normal  transient 
analysis LS-DYNA continues the output of data as it would without the dynam-
ic  relaxation  being  active.    This  is  unlike  the  dynamic  relaxation  phase  at  the 
beginning  of  the  calculation  when  a  separate  database  is  not  used.    Only  load 
curves that are flagged for dynamic relaxation are applied after restarting.
*CONTROL_SHELL 
Purpose:    Change  failure  parameters  NFAIL1  and  NFAIL4    if  necessary.    These 
parameters must be nonzero in the initial run. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
  VARIABLE   
NFAIL1 
NFAIL1 
NFAIL4 
PSNFAIL 
I 
I 
I 
DESCRIPTION
Flag to check for highly distorted under-integrated shell elements, 
print a message, and delete the element or terminate.  Generally,
this flag is not needed for one point elements that do not use the
warping  stiffness.    A  distorted  element  is  one  where  a  negative 
jacobian  exists  within  the  domain  of  the  shell,  not  just  at
  The  checks  are  made  away  from  the
integration  points. 
integration points to enable the bad elements to be deleted before
an instability leading to an error termination occurs.  This test will 
increase CPU requirements for one point elements. 
EQ.1: print message and delete element. 
EQ.2: print message, write d3dump file, and terminate 
GT.2: print  message  and  delete  element.    When  NFAIL1
elements  are  deleted  then  write  D3dump  file  and  termi-
nate.  These NFAIL1 failed elements also include all shell
elements  that  failed  for  other  reasons  than  distortion.
Before the d3dump file is written, NFAIL1 is doubled, so 
the run can immediately be continued if desired.
VARIABLE   
NFAIL4 
DESCRIPTION
Flag to check for highly distorted fully-integrated shell elements, 
print a message, and delete the element or terminate.  Generally,
this  flag  is  recommended.      A  distorted  element  is  one  where  a
negative jacobian exists within the domain of the shell, not just at
integration points. 
The  checks  are  made  away  from  the  integration  points to  enable
the bad elements to be deleted before an instability leading to an
error termination occurs. 
EQ.1: print message and delete element.   
EQ.2: print message, write d3dump file, and terminate 
GT.2: print  message  and  delete  element.    When  NFAIL4
elements  are  deleted  then  write  d3dump  file  and  termi-
nate.  These NFAIL4 failed elements also include all shell
elements  that  failed  for  other  reasons  than  distortion.
Before the d3dump file is written, NFAIL4 is doubled, so 
the run can immediately be continued if desired. 
PSNFAIL 
Optional  shell  part  set  ID  specifying  which  part  IDs  are  checked
by the NFAIL1, NFAIL4, and W-MODE options.  If zero, all shell 
part IDs are included.
*CONTROL_TERMINATION 
Purpose:  Stop the job. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ENDTIM 
ENDCYC 
Type 
F 
I 
  VARIABLE   
DESCRIPTION
ENDTIM 
Termination time: 
EQ.0.0: Termination time remains unchanged. 
ENDCYC 
Termination cycle.  The termination cycle is optional and will be
used if the specified cycle is reached before the termination time. 
EQ.0.0: Termination cycle remains unchanged. 
Remarks: 
This  is  a  reduced  version  of  the  *CONTROL_TERMINATION  card  used  in  the  initial 
input deck.
RESTART INPUT DATA 
Purpose:  Set time step size control using different options. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DUMMY 
tssfac 
ISDO 
DUMMY 
DT2MS 
LCTM 
Type 
F 
F 
I 
F 
F 
I 
  VARIABLE   
DESCRIPTION
DUMMY 
Dummy field, see remark 1 below. 
TSSFAC 
Scale factor for computed time step. 
EQ.0.0: TSSFAC remains unchanged. 
ISDO 
Basis  of  time  size  calculation  for  4-node  shell  elements,  ISDO  3-
node  shells  use  the  shortest  altitude  for  options  0,1  and  the
shortest  side  for  option  2.    This  option  has  no  relevance  to  solid
elements,  which  use  a  length  based  on  the  element  volume
divided by the largest surface area: 
EQ.0: characteristic length = area/(longest side), 
EQ.1: characteristic length = area/(longest diagonal), 
EQ.2: based  on  bar  wave  speed  and  MAX  [shortest  side,
area/longest  side].    THIS  LAST  OPTION  CAN  GIVE  A 
MUCH  LARGER  TIME  STEP  SIZE  THAT  CAN  LEAD
TO  INSTABILITIES  IN  SOME  APPLICATIONS,  ESPE-
CIALLY WHEN TRIANGULAR ELEMENTS ARE USED.
DUMMY 
Dummy field, see remark 1 below. 
DT2MS 
New time step for mass scaled calculations.  Mass scaling must be
active in the time zero analysis. 
EQ.0.0: DT2MS remains unchanged. 
LCTM 
Load curve ID that limits maximum time step size: 
EQ.0: LCTM remains unchanged.
Remarks: 
1.  This  a  reduced  version  of  the  *CONTROL_TIMESTEP  used  in  the  initial 
analysis.    The  dummy  fields  are  included  to  maintain  compatibility.    If  using 
free format input then a 0.0 should be entered for the dummy values.
RESTART INPUT DATA 
Purpose:  Define mass weighted nodal damping that applies globally to the deformable 
nodes. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
VALDMP 
Type 
Default 
I 
0 
F 
0.0 
  VARIABLE   
DESCRIPTION
LCID 
Load curve ID which specifies node system damping: 
EQ.n: system damping is given by load curve n.  The damping
force  applied  to  each  node  is  f = -d(t)  mv,  where  d(t)  is 
defined by load curve n. 
VALDMP 
System  damping  constant,  d  (this  option  is  bypassed  if  the  load
curve number defined above is nonzero).
*DATABASE_OPTION 
Options  for  ASCII  files  include.    If  a  file  is  not  specified  in  the  restart  deck  then  the 
output interval for the file will remain unchanged. 
SECFORC  Cross section forces. 
RWFORC  Wall forces. 
NODOUT  Nodal point data. 
ELOUT  
Element data. 
GLSTAT 
Global data. 
DEFORC  Discrete elements. 
MATSUM  Material energies. 
NCFORC  Nodal interface forces. 
RCFORC 
Resultant interface forces. 
DEFGEO  Deformed geometry file 
SPCFORC  Set dt for spc reaction forces. 
SWFORC  Nodal constraint reaction forces (spot welds and rivets). 
ABSTAT 
Set dt for airbag statistics. 
NODFOR 
Set dt for nodal force groups. 
BNDOUT  Boundary condition forces and energy  
RBDOUT   Set dt for rigid body data. 
GCEOUT  
Set dt for geometric contact entities. 
SLEOUT 
Set dt for sliding interface energy. 
JNTFORC  Set dt for joint force file. 
SBTOUT 
Set dt for seat belt output file. 
AVSFLT 
Set dt for AVS database. 
MOVIE 
Set dt for MOVIE. 
MPGS 
Set dt for MPGS. 
TPRINT 
Set dt for thermal file.
RESTART INPUT DATA 
2 
3 
4 
5 
6 
7 
8 
*DATABASE 
Card 
Variable 
1 
DT 
Type 
F 
  VARIABLE   
DESCRIPTION
DT 
Time interval between outputs: 
EQ.0.0: output interval is unchanged. 
Remarks: 
To terminate output to a particular file set DT to a high value. 
If IACCOP = 2 was specified in *CONTROL_OUTPUT, the best results are obtained in 
the NODOUT file by keeping the same DT on restart.  When DT is changed for NOD-
OUT,  oscillations  may  occur  around  the  restart  time.    If  DT  is  larger  than  initially 
specified in the original input file, more memory is required to store the time states for 
the  averaging  than  was  originally  allocated.    A  warning  message  is  printed,  and  the 
filtering  is  applied  using  the  available  memory.    When  DT  is  smaller  than  initially 
specified,  more  oscillations  may  appear  in  the  output  than  earlier  in  the  calculation 
because the frequency content of the averaged output increases as DT decreases.
*DATABASE_BINARY 
Options for binary output files with the default names given include: 
D3PLOT 
Dt for complete output states. 
D3THDT  Dt for time history data for element subsets. 
D3DUMP  Binary output restart files.  Define output frequency in cycles 
RUNRSF  
Binary output restart file.  Define output frequency in cycles. 
INTFOR 
Dt for contact surface Interface database. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  DT/CYCL 
Type 
F 
  VARIABLE   
DESCRIPTION
DT 
Time interval between outputs. 
EQ.0.0: Time interval remains unchanged. 
CYCL 
Output interval in time steps. 
EQ.0.0: output interval remains unchanged.
*DELETE_OPTION 
Available options are: 
ALECPL 
CONTACT 
CONTACT_2DAUTO 
ENTITY 
PART 
ELEMENT_BEAM 
ELEMENT_SHELL 
ELEMENT_SOLID 
ELEMENT_TSHELL 
FSI 
Purpose:  Delete contact surfaces, ALE FSI couplings, parts, or elements by a list of IDs.  
There are two contact algorithms for two-dimensional problems: the line-to-line contact 
and the automatic contact defined by part ID's.  Each uses their own numbering. 
  This 
ID  Cards. 
the  ALECPL,  CONTACT, 
format  applies 
CONTACT_2DAUTO,  ENTITY,  FSI  and  PART  options.    Include  as  many  cards  as 
necessary to input desired IDs.  This input ends at the next keyword (“*”) card. 
card  1 
to 
Card 
1 
Variable 
ID1 
2 
ID2 
3 
ID3 
4 
ID4 
5 
ID5 
6 
ID6 
7 
ID7 
8 
ID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
  VARIABLE   
DESCRIPTION
IDn 
Contact ID/Coupling ID/Part ID 
Remarks: 
The  FSI  option  corresponds  to  ALE  couplings  defined  with  *CONSTRAINED_LA-
GRANGE_IN_SOLID.      The  ALECPL  option  corresponds  to  ALE  couplings  defined
with  *ALE_COUPLING_NODAL_CONSTRAINT.    For  CONTACT,  FSI,  and  ALECPL 
options,  a  negative  ID  implies  that  the  absolute  value  gives  the  contact  sur-
face/FSI/ALECPL coupling which is to be activated. 
Element  set  cards.    This  card  1  format  applies  to  the  four  ELEMENT  options.    This 
input ends at the next keyword (“*”) card. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ESID 
Type 
I 
  VARIABLE   
ESID 
DESCRIPTION
Element  set  ID,  see  *SET_SOLID,  *SET_BEAM,  *SET_SHELL, 
*SET_TSHELL.
*INTERFACE_SPRINGBACK_LSDYNA 
Purpose:  Define a material subset for output to a stress initialization file “dynain”.  The 
dynain  file  contains  keyword  commands  that  can  be  included  in  a  subsequent  input 
deck  to  initialize  deformation,  stress,  and  strain  in  parts.    This  file  can  be  used,  for 
example, to do an implicit springback analysis after an explicit forming analysis. 
Part Set ID Cards. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PSID 
NSHV 
Type 
I 
I 
Constraint Cards.  Optional cards that list of nodal points that are constrained in the 
dynain file.  This input ends at the next keyword (“*”) card. 
4 
5 
6 
7 
8 
  Card 2 
1 
Variable 
NID 
Type 
I 
2 
TC 
F 
Default 
none 
0. 
3 
RC 
F 
0. 
  VARIABLE   
DESCRIPTION
PSID 
NSHV 
Part set ID for springback, see *SET_PART. 
  If  NSHV 
Number of shell or solid history variables (beyond the six stresses
and  effective  plastic  strain)  to  be  initialized  in  the  interface  file.
For  solids,  one  additional  state  variable  (initial  volume)  is  also
written. 
is  nonzero,  the  element  formulations,
calculational  units,  and  constitutive  models  should  not  change
between runs.  If NHSV exceeds the number of integration point
history  variables  required  by  the  constitutive  model,  only  the
number  required  is  written;  therefore,  if  in  doubt,  set  NHSV  to
alarge number. 
NID 
Node ID
VARIABLE   
DESCRIPTION
TC 
Translational constraint: 
EQ.0: no constraints, 
EQ.1: constrained x displacement, 
EQ.2: constrained y displacement, 
EQ.3: constrained z displacement, 
EQ.4: constrained x and y displacements, 
EQ.5: constrained y and z displacements, 
EQ.6: constrained z and x displacements, 
EQ.7: constrained x, y, and z displacements. 
RC 
Rotational constraint: 
EQ.0: no constraints, 
EQ.1: constrained x rotation, 
EQ.2: constrained y rotation, 
EQ.3: constrained z rotation, 
EQ.4: constrained x and y rotations, 
EQ.5: constrained y and z rotations, 
EQ.6: constrained z and x rotations, 
EQ.7: constrained x, y, and z rotations.
*RIGID_DEFORMABLE_OPTION 
Available options include: 
CONTROL 
D2R                  (Deformable to rigid part switch)  
R2D                  (Rigid to deformable part switch) 
Purpose:  Define parts to be switched from rigid to deformable and deformable to rigid 
in a restart.  It is only possible to switch parts on a restart if part switching was activated 
in the time zero analysis.  See *DEFORMABLE_TO_RIGID for details of part switching.
*RIGID_DEFORMABLE_CONTROL 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NRBF 
NCSF 
RWF 
DTMAX 
Type 
Default 
I 
0 
I 
0 
I 
0 
F 
none 
  VARIABLE   
NRBF 
DESCRIPTION
Flag to delete or activate nodal rigid bodies. 
If nodal rigid bodies or generalized, weld definitions are active in 
the  deformable  bodies  that  are  switched  to  rigid,  then  the
definitions should be deleted to avoid instabilities: 
EQ.0: no change, 
EQ.1: delete, 
EQ.2: activate. 
NCSF 
Flag to delete or activate nodal constraint set. 
If  nodal  constraint/spot  weld  definitions  are  active  in  the
deformable bodies that are switched to rigid, then the definitions
should be deleted to avoid instabilities: 
EQ.0: no change, 
EQ.1: delete, 
EQ.2: activate. 
RWF 
Flag to delete or activate rigid walls: 
EQ.0: no change, 
EQ.1: delete, 
EQ.2: activate. 
DTMAX 
Maximum permitted time step size after restart.
*RIGID_DEFORMABLE_D2R 
Part  ID  Cards.    Include  one  card  for  each  part.    This  input  ends  at  the  next  keyword 
(“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
MRB 
Type 
I 
Default 
none 
I 
0 
  VARIABLE   
DESCRIPTION
PID 
MRB 
Part ID of the part which is switched to a rigid material. 
Part ID of the master rigid body to which the part is merged.  If
zero,  the  part  becomes  either  an  independent  or  master  rigid
body.
*RIGID_DEFORMABLE_R2D 
Termination of this input is when the next “*” card is read. 
Part  ID  Cards.    Include  one  card  for  each  part.    This  input  ends  at  the  next  keyword 
(“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
Type 
I 
Default 
none 
  VARIABLE   
DESCRIPTION
PID 
Part ID of the part which is switched to a deformable material.
*STRESS_INITIALIZATION_{OPTION} 
This keyword causes a full deck restart.  For a full deck restart the input deck must contain 
the  full  model.    The  stress  initialization  feature  allows  all  or  selected  parts  to  be 
initialized  from  the  previous  calculation  using  data  from  the  d3dump  or  runrsf 
databases. 
The options that are available with this keyword are: 
<BLANK> 
DISCRETE 
SEATBELT 
Optional Part Cards.  If no part cards are included in the deck then all parts, seatbelts 
and discrete parts in the new input deck that existed in the previous input deck (with or 
without  the  same  part  IDs)  are  initialized  from  the  d3dump  or  runrsf  database. 
Otherwise for each part to be initialized from the restart data include an addition card 
in format 1.  This input terminates at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PIDO 
PIDN 
Type 
I 
I 
Default 
none 
PIDO 
  VARIABLE   
DESCRIPTION
PIDO 
PIDN 
Old part ID, see *PART. 
New part ID, see *PART: 
EQ.0: New part ID is the same as the old part ID. 
Remarks: 
If  one  or  more  of  the  above  cards  are  defined  then  discrete  and  seatbelt  elements  will 
not  be  initialized  unless  the  additional  option  cards  *STRESS_INITIALIZATION_DIS-
CRETE and *STRESS_INITIALIZATION_SEATBELT are defined. 
*STRESS_INITIALIZATION_DISCRETE
Initialize  all  discrete  parts  from  the  old  parts.    No  further  input  is  required  with  this 
card.    This  card  is  not  required  if  *STRESS_INITIALIZATION  is  specified  without 
further input. 
*STRESS_INITIALIZATION_SEATBELT 
Initialize  all  seatbelt  parts  from  the  old  parts.    No  further  input  is  required  with  this 
card.    This  card  is  not  required  if  *STRESS_INITIALIZATION  is  specified  without 
further input.
RESTART INPUT DATA 
Purpose:  Stops the job depending on some displacement conditions. 
Available options include: 
NODE 
BODY 
Caution:  The  inputs  are  different  for  the  nodal  and  rigid  body  stop  conditions.    The 
nodal  stop  condition  works  on  the  global  coordinate  position,  while  the  body  stop 
condition  works  on  the  relative  global  translation.    The  number  of  termination 
conditions  cannot  exceed  the  maximum  of  10  or  the  number  specified  in  the  original 
analysis.   
The  analysis  terminates  for  *TERMINATION_NODE  when  the  current  position  of  the 
node specified reaches either the maximum or minimum value (stops 1, 2 or 3), or picks 
up  force  from  any  contact  surface  (stop  4).    For  *TERMINATION_BODY  the  analysis 
terminates  when  the  center  of  mass  displacement  of  the  rigid  body  specified  reaches 
either the maximum or minimum value (stops 1, 2 or 3) or the displacement magnitude 
of  the  center  of  mass  is  exceeded  (stop  4).    If  more  than  one  condition  is  input,  the 
analysis stops when any of the conditions is satisfied. 
NOTE:  This  input  completely  overrides  the  existing  termi-
nation conditions defined in the time zero run. 
Termination  by other means  is  controlled  by  the  *CONTROL_TERMINATION  control 
card.
Node/Part Cards.  Include an additional card in format 1 for each node or part with a 
termination criterion 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID/PID 
STOP 
MAXC 
MINC 
Type 
I 
I 
Default 
none 
none 
F 
- 
F 
- 
For the NODE option: 
  VARIABLE   
DESCRIPTION
NID 
STOP 
Node ID 
Stop criterion: 
EQ.1: global x direction, 
EQ.2: global y direction, 
EQ.3: global z direction, 
EQ.4: stop if node touches contact surface. 
MAXC 
MINC 
Maximum  (most  positive)  coordinate,  options  1,  2  and  3  above
only. 
Minimum  (most  negative)  coordinate,  options  1,  2  and  3  above
only. 
For the BODY option: 
  VARIABLE   
DESCRIPTION
PID 
Part ID of rigid body
VARIABLE   
DESCRIPTION
STOP 
Stop criterion: 
EQ.1: global x direction, 
EQ.2: global y direction, 
EQ.3: global z direction, 
EQ.4: stop if displacement magnitude is exceeded. 
MAXC 
Maximum (most positive) displacement, options 1, 2, 3 and 4: 
EQ.0.0: MAXC set to 1.0e21 
MINC 
Minimum (most negative) displacement, options 1, 2 and 3 above
only: 
EQ.0.0: MINC set to -1.0e21
*TITLE 
Purpose:  Define job title. 
Card 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
TITLE 
C 
LS-DYNA USER INPUT 
  VARIABLE   
DESCRIPTION
TITLE 
Heading to appear on output.
REFERENCES 
REFERENCES 
Abbo,  A.J.,  and  S.W.    Sloan,  “A  Smooth  Hyperbolic  Approximation  to  the  Mohr-
Coulomb Yield Criterioin,” Computers and Structures, Vol.  54, No.  1, (1995). 
Allen,  D.J.,  Rule,  W.K.,  Jones,  S.E.,  “Optimizing  Material  Strength  Constants 
Numerically  Extracted  from  Taylor  Impact  Data”,  Experimental  Mechanics,  Vol.  
37, No 3, September (1997). 
Allman,  D.J.,  “A  Compatible  Triangular  Element  Including  Vertex  Rotations  for  Plane 
Elasticity Analysis,” Computers and Structures, 19, 1-8, (1984). 
Anagonye,  A.U.    and  J.T.    Wang,  “A  Semi-Empirical  Method  for  Estimating  the 
Effective Leak and Vent Areas of an Airbag”, AMD-Vol.  237/BED-Vol.  45, pp.  
195-217, (1999). 
Anand,  L.    and  M.E.    Gurtin,  “A  theory  of  amorphous  solids  undergoing  large 
deformations,  with  application  to  polymeric  glasses,”  International  Journal  of 
Solids and Structures, 40, pp.  1465-1487 (2003) 
Aretz, H.  “Applications of a New Plane Stress Yield Function to Orthotropic Steel and 
Aluminum  Sheet  Metals,”  Modeling  and  Simulation  in  Materials  Science  and 
Engineering, 12, 491-509 (2004). 
Argon, AS., “A theory for the low-temperature plastic deformation of glassy polymers”, 
Philosophical Magazine, 28, 839-865 (1973). 
Armstrong, P.J., and Frederick, C.O., “A Mathematical Representation of the Multiaxial 
Bauschinger  Effect,”  CEGB  Report,  RD/B/N731,  Berkeley  Nuclear  Laboratories 
(1966).   
Arruda,  E.    and  M.    Boyce,  “A  Three-Dimensional  Constitutive  Model  for  the  Large 
Stretch Behavior of Rubber Elastic Materials,” Journal of the Mechanics and Physics 
of Solids, Vol.  41, No.  2, pp.  389-412, (1993). 
Auricchio, F., R.L.  Taylor and J.  Lubliner, “Shape-memory alloys: macromodeling and 
numerical simulations of the superelastic behavior”, Computer Methods in Applied 
Mechanics and Engineering, vol.  146, pp.  281-312, (1997). 
Auricchio,  F.    and  R.L.    Taylor,  “Shape-memory  alloys:  modeling  and  numerical 
simulations  of  the  finite-strain  superelastic  behavior”,  Computer  Methods  in 
Applied Mechanics and Engineering, vol.  143, pp.  175-194, (1997). 
Bahler  AS:    The  series  elastic  element  of  mammalian  skeletal  muscle.    Am  J  Physiol 
213:1560-1564, (1967).
REFERENCES 
Baker,  E.L.,  “An  Explosives  Products  Thermodynamic  Equation  of  State  Appropriate 
for  Material  Acceleration  and  Overdriven  Detonation:  Theoretical  Background 
and Fourmulation,” Technical Report ARAED-TR-911013, U.S.  Army Armament 
Research, Development and Engineering Center, Picatinney Arsenal, New Jersey, 
1991). 
Baker, E.L.  and J.  Orosz, J., “Advanced Warheads Concepts: An Advanced Equation of 
State  for  Overdriven  Detonation,”  Technical  Report  ARAED-TR-911007,  U.S.  
Army  Armament  Research,  Development  and  Engineering  Center,  Picatinney 
Arsenal, New Jersey, (1991). 
Baker,  E.L.    and  L.I.    Stiel,  “Improved  Quantitative  Explosive  Performance  Prediction 
Using  Jaguar,”  1997  Insensitive  Munitions  and  Energetic  Materials  Technology 
Symposium, Tampa, FL, (1997). 
Bammann,  D.J.    and  E.C.    Aifantis,  “A  Model  for  Finite-Deformation  Plasticity,”  Acta 
Mechanica, 70, 1-13 (1987). 
Bammann, D.J.  and G.  Johnson, “On the Kinematics of Finite-Deformation Plasticity,” 
Acta Mechanica, 69, 97-117 (1987). 
Bammann,  D.J.,  “Modeling  the  Temperature  and  Strain  Rate  Dependent  Large 
Deformation  of  Metals,”  Proceedings  of  the  11th  US  National  Congress  of 
Applied Mechanics, Tuscon, AZ, (1989). 
Bammann,  D.J.,  M.L.    Chiesa,  A.    McDonald,  W.A.    Kawahara,  J.J.    Dike,  and  V.D.  
Revelli,  “Predictions  of  Ductile  Failure  in  Metal  Structures,”  in  AMD-Vol.    107, 
Failure Criteria and Analysis in Dynamic Response, Edited by.  H.E.  Lindberg, 
7-12, (1990). 
Bandak, F.A., private communications, U.S.  Dept.  of Trans., Division of Biomechanics 
Research, 400 7th St., S.W.  Washington, D.C.  20590 (1991). 
Bansal,  S.,  Mobasher,  B.,  Rajan,  S.,  and  Vintilescu,  I.,  “Development  of  Fabric 
Constitutive  Behavior  for  Use  in  Modeling  Engine  Fan  Blade-Out  Events.”  J.  
Aerosp.    Eng.    22,  SPECIAL  ISSUE:  Ballistic  Impact  and  Crashworthiness 
Response of Aerospace Structures, 249–259, (2009). 
Barlat,  F.    and  J.    Lian,  “Plastic  Behavior  and  Stretchability  of  Sheet  Metals.    Part  I:  A 
Yield Function for Orthotropic Sheets Under Plane Stress Conditions,” Int.  J.  of 
Plasticity, Vol.  5, pp.  51-66 (1989). 
Barlat, F., D.J.  Lege, and J.C.  Brem, “A Six-Component Yield Function for Anisotropic 
Materials,” Int.  J.  of Plasticity, 7, 693-712, (1991). 
Barlat, F., Y.  Maeda, K.  Chung, M.  Yanagawa, J.C.  Brem, Y.  Hayashida, D.J.  Lege, K.  
Matsui, S.J.  Murtha, S.  Hattori, R.C.  Becker, and S.  Makosey, “Yield Function
REFERENCES 
Development for Aluminum Alloy Sheets”, J.  Mech.  Phys.  Solids, Vol.  45, No.  
11-12, 1727-1763, (1997). 
Barlat, F., Brem, J.C., Yoon, J.W., Chung, K., Dick, R.E., Lege, D.J., Pourboghrat, F., Choi, 
S.H., Chu, E., “Plane Stress Yield Function for Aluminum Alloy Sheets – Part 1: 
Theory, Int.  J.  Plast.  19, 1-23, (2003).  
Basu,  U.,  “Explicit  finite  element  perfectly  matched  layer  for  transient  three-
dimensional  elastic  waves,”  International  Journal  for  Numerical  Methods  in 
Engineering, vol.  77, pp.  151–176, (2009).  
Basu,  U. 
  and  Chopra,  A.K.,  “Perfectly  matched 
time-harmonic 
elastodynamics 
finite-element 
implementation,”  Computer  Methods  in  Applied  Mechanics  and  Engineering,  vol.  
192, pp.  1337–1375, (2003). 
of  unbounded  domains 
for 
and 
theory 
layers 
Basu,  U.    and  Chopra,  A.K.,  “Perfectly  matched  layers  for  transient  elastodynamics  of 
unbounded  domains,”  International  Journal  for  Numerical  Methods  in  Engineering, 
vol.  59, pp.  1039–1074, (2004).  Erratum: Ibid.  vol.  61, pp.  156–157, (2004). 
Bathe,  K.-J.    Conserving  energy  and  momentum  in  nonlinear  dynamics:  A  simple 
implicit time integration scheme, Computers and Structures, 85, 437-445 (2007). 
Bathe, K.-J.  and Dvorkin, E.N.  A four node plate bending element based on Mindlin-
Reissner  plate  theory  and  a  mixed  interpolation,  Int.    J.    Num.    Meth.    Eng.,  21, 
367-383 (1985). 
Bathe, K-J.  and Nooh, G. Insight into an implicit time integration scheme for structural 
dynamics, Computers and Structures, 98/99, 1-6 (2012). 
Batoz,  J.L.    and  Ben  Tahar,  M.    Evaluation  of  a  new  quadrilateral  thin  plate  bending 
element, Int. J.  Num.  Meth.  Eng., 18, 1644-1677 (1982). 
Batoz,  J.-L.    and  M.    Ben  Tahar,  Evaluation  of  a  new  quadrilateral  thin  plate  bending 
element,  International  Journal  for  Numerical  Methods  in  Engineering,  18,  (1982), 
1655-1677. 
Bazeley, G.P., W.K.  Cheung, R.M.  Irons, and O.C.  Zienkiewicz, “Triangular Elements 
in  Plate  Bending-Confirming  and  Nonconforming  Solutions  in  Matrix  Methods 
and  Structural  Mechanics,”  Proc.    Conf.    on  Matrix  Methods  in  Structural 
Analysis, Rept.  AFFDL-R-66-80, Wright Patterson AFB, 547-576 (1965). 
Belytschko, T.  and Bindeman, L.  P.  “Assumed Strain Stabilization of the Eight Node 
Hexahedral Element,” Comp.  Meth.  Appl.  Mech.  Eng. 105, 225-260 (1993).
REFERENCES 
Belytschko,  T.B.    and  A.H.    Marchertas,  “Nonlinear  Finite  Element  Method  for  Plates 
and  its  Application  to  the  Dynamic  Response  of  Reactor  Fuel  Subassemblies,” 
Trans, ASME J.  Pressure Vessel Tech., 251-257 (1974). 
Belytschko,  T.B.    and  C.S.    Tsay,  “Explicit  Algorithms  for  Nonlinear  Dynamics  of 
Shells,” AMD-Vol.48, ASME, 209-231 (1981). 
Belytschko,  T.B.    and  C.S.    Tsay,  “Explicit  Algorithms  for  Nonlinear  Dynamics  of 
Shells,” Comp.  Meth.  Appl.  Mech.  Eng., 43, 251-276, (1984). 
Belytschko, T.B.  and C.S.  Tsay, “A Stabilization Procedure for the Quadrilateral Plate 
Element  with  One-Point  Quadrature,”  Int.    J.    Num.    Method.    Eng.,  19,  405-419 
(1983). 
Belytschko, T.B., H.  Stolarski, and N.  Carpenter, “A C° Triangular Plate Element with 
One-Point Quadrature,” Int.  J.  Num.  Meth.  Eng., 20, 787-802 (1984). 
Belytschko, T.B., I.  Yeh, “The Splitting Pinball Method for Contact-Impact Problems,” 
Comp.  Meth.  Appl.  Mech.  Eng., 105, 375-393, (1993). 
Belytschko, T.B., L.  Schwer, and M.J.  Klein, “Large Displacement Transient Analysis of 
Space Frames,” Int.  J.  Num.  Eng., 11, 65-84 (1977). 
Benson,  D.J.    and  J.O.    Hallquist,  “A  Simple  Rigid  Body  Algorithm  for  Structural 
Dynamics Programs,” Int.  J.  Numer.  Meth.  Eng., 22, (1986). 
Benson,  D.J.    and  J.O.    Hallquist,  “A  Single  Surface  Contact  Algorithm  for  the 
Postbuckling  Analysis  of  Shell  Structures,”  Comp.    Meths.    Appl.    Mech.    Eng., 
78, 141-163 (1990). 
Benzeggagh,  M.L.    and  Kenane,  M.,  “Measurement  of  Mixed-mode  Delamination 
Fracture  Toughness  of  Unidirectional  Glass/Epoxy  Composites  with  Mixed-
mode  Bending  Apparatus,”  Composites  Science  and  Technology,  56,  439-449 
(1996).  
Berstad,  T.,  “Material Modeling  of  Aluminium  for  Crashworthiness  Analysis”,  Dr.Ing.  
Dissertation,  Department  of  Structural  Engineering,  Norwegian  University  of 
Science and Technology, Trondheim, Norway, (1996). 
Berstad,  T.,  Hopperstad,  O.S.,  Lademo,  O.-G.    and  Malo,  K.A.,  “Computational  Model 
of Ductile Damage and Fracture in Shell Analysis”, Second European LS-DYNA 
Conference, Gothenburg, Sweden, (1999). 
Berstad, T., Lademo, O.-G., Pedersen, K.O.  and Hopperstad, O.S., “Formability modeling 
with LS-DYNA”, 8th International LS-DYNA User’s Conference, Detroit, May 3-5, 
2004.
REFERENCES 
Berstad,  T.,  Langseth,  M.    and  Hopperstad,  O.S.,  “Elasto-viscoplastic  Constitutive 
Models in the Explicit Finite Element Code LS-DYNA3D,” Second International 
LS-DYNA3D conference, San Francisco, (1994). 
Bergström,  J.S.    and  M.C.    Boyce,  “Constitutive  modeling  of  the  large  strain  time-
dependent behavior of elastomers” J.  Mech.  Phys.  Solids, 46, 931-954 (1998). 
Bielak, J.  and Christiano, P., “On the effective seismic input for non-linear soil-structure 
interaction systems,” Earthquake Engineering and Structural Dynamics, vol.  12, pp.  
107–119, (1984). 
Bier,  M.,  Sommer,  S.,  “Simplified  modeling  of  self-piercing  riveted  joints  for  crash 
simulation 
of 
*CONSTRAINED_INTERPOLATION_SPOTWELD”.    9th  European  LS-DYNA 
Conference, Manchester, (2013). 
modified 
version 
with 
a 
Bilkhu, S.S., M.  Founas, and G.S.  Nasholtz, “Material Modeling of Structural Foams in 
Finite  Element  Analysis  Using  Compressive  Uniaxial  and  Triaxial  Data,”  SAE 
(Nat.  Conf.) Detroit 1993, pp.  4-34. 
Blatz,  P.J.,  and  Ko,  W.L.,  “Application  of Finite  Element  Theory  to the  Deformation  of 
Rubbery Materials,” Trans.  Soc.  of Rheology, 6, 223-251 (1962). 
Borrvall T., Bhalsod D., Hallquist J.O., and Wainscott B., “Current Status of Subcycling 
and  Multiscale  Simulations  in  LS-DYNA”.    13th  International  LS-DYNA  User’s 
Conference, Dearborn MI, (2014). 
Boyce,  M.C.,  Parks,  D.M.,  and  Argon,  A.S.,  “Large  inelastic  deformation  of  glassy 
polymers.  Part I: Rate dependent constitutive model”. Mechanics of Materials, 7, 
15-33 (1988). 
Boyce, M.C., Socrate, C.  and Llana, P.G., “Constitutive model for the finite deformation 
stress-strain behavior of poly(ethylene terephthalate) above the glass transition”. 
Polymer, 41, 2183-2201 (2000). 
Brandt,  J.,  On  Constitutive  Modelling  of  the  Compaction  and  Sintering  of  Cemented 
Carbides, Linköping Studies in Science and Technology, Dissertations 515, 1998. 
Brekelmans,  W.A.M.,  Scheurs,P.J.G.,  and  de  Vree,  J.H.P.,  1991,  “Continuum  damage 
mechanics for softening of brittle materials”, Acta Mechanica, vol 93, pp 133-143 
Broadhouse,  B.J.,  “The  Winfrith  Concrete  Model 
in  LS-DYNA3D,”  Report: 
SPD/D(95)363,  Structural  Performance  Department,  AEA  Technology,  Winfrith 
Technology Centre, U.K.  (1995).
REFERENCES 
Broadhouse,  B.J.    and  Neilson,  A.J.,  “Modelling  Reinforced  Concrete  Structures  in 
DYNA3D”,  Safety  and  Engineering  Division,  United  Kingdom  Atomic  Energy 
Authority, Winfrith, AEEW-M 2465, 1987. 
Brode,  H.L.,  “Height  of  Burst  Effects  at  High  Overpressure,”  RAND,  RM-6301-DASA, 
DASA 2506, (1970). 
Brown,  B.E.    and  J.O.    Hallquist,  “TAURUS:  An  Interactive  Post-Processor  for  the 
Analysis  Codes  NIKE3D,  DYNA3D,  TACO3D,  and  GEMINI,”  University  of 
California,  Lawrence  Livermore  National  Laboratory,  Rept.    UCID-19392  (1982) 
Rev.  1 (1984). 
Bruneau,  M.,  Uang,  C.M.,  Whittaker,  A.,  Ductile  Design  of  Steel  Structures,  McGraw 
Hill, (1998).  
Burton, D.E.  et al.  “Physics and Numerics of the TENSOR Code,” Lawrence Livermore 
National Laboratory, Internal Document UCID-19428, (July 1982).  
Carney,  K.S.,  S.A.    Howard,  B.A.    Miller,  and  D.J.    Benson.    “New  Representation  of 
in  LS-DYNA,”  13th  International  LS-DYNA  Users  Conference, 
Bearings 
Dearborn, MI, June 8-10, 2014. 
CEB Code 1993, Comite euro-international du beton, CEB-FIP Model Code 1990, Thomas 
Telford, London, (1993). 
Chang,  F.K.    and  K.Y.    Chang,  “A  Progressive  Damage  Model  for  Laminated 
Composites Containing Stress Concentration,” J.   of Composite  Materials, 21, 834-
855 (1987a). 
Chang,  F.K.    and  K.Y.    Chang,  “Post-Failure  Analysis  of  Bolted  Composite  Joints  in 
Tension or Shear-Out Mode Failure,” J.  of Composite Materials, 21 809-823 (1987b). 
Chang,  F.S.,  “Constitutive  Equation  Development  of  Foam  Materials,”  Ph.D.  
Dissertation, submitted to the Graduate School, Wayne State University, Detroit, 
Michigan (1995). 
Chao, Y.  J., Wang, K, Miller, K.  W.  and Zhu, X.  K.  “Dynamic Separation of Resistance 
Spot Welded joints: Part I – Experiments”, Exp Mech, Vol.  50, Issue 7, pp 889-900 
(2010). 
Chen, W.F., and Baladi, G.Y., Soil Plasticity: Theory and Implementation, Elesvier, New 
York, (1985). 
Cheng,  H.,  Obergefell,  L.A.,  and  Rizer,  A.,  March  1994,  “Generator  of  Body  (GEBOD) 
Manual,” Report No.  AL/CF-TR-1994-0051.
REFERENCES 
Chowdhury,  S.R.    and  Narasimhan  R.,  “A  Cohesive  Finite  Element  Formulation  for 
Modeling Fracture and Delamination in Solids,” Sadhana, 25(6), 561-587, (2000).   
Christensen,  R.M. 
  “A  Nonlinear  Theory  of  Viscoelasticity  for  Application  to 
Elastomers,”  Journal  of  Applied  Mechanics,  Volume  47,  American  Society  of 
Mechanical Engineers, pages 762-768, December 1980. 
Chu, C.C.  and A.  Needleman, “Void Nucleation Effects in Biaxially Stretched Sheets”, 
ASME Journal of Engineering Materials and Technology, 102, 249-256 (1980). 
Chung, K.  and K.  Shah, “Finite Element Simulation of Sheet Metal Forming for Planar 
Anisotropic Metals,” Int.  J.  of Plasticity, 8, 453-476, (1992). 
Cochran, S.G.  and J.  Chan, “Shock Initiation and Detonation Models in One and Two 
Dimensions,”  University  of  California,  Lawrence  Livermore  National 
Laboratory, Rept.  UCID-18024 (1979). 
Cook,  R.    D.,  Concepts  and  Applications  of  Finite  Element  Analysis,  John  Wiley  and 
Sons, Inc.  (1974). 
Couch,  R.,  E.    Albright,  and  N.    Alexander,  The  Joy  Computer  Code,  Lawrence 
Livermore National Laboratory, Internal Document Rept.  UCID-19688, (January, 
1983). 
Cowper,  G.R.    and  P.S.    Symonds,  Strain  Hardening  and  Strain  Rate  Effects  in  the 
Impact  Loading  of  Cantilever  Beams,  Brown  University,  Applied  Mathematics 
Report, 1958. 
CRAY-1  Computer  System  CFT  Reference  Manual,  Cray  Research  Incorporated, 
Bloomington, NM., Publication No.  2240009 (1978). 
Dal,  H.    and  M.    Kaliske,  “Bergström-Boyce  model  for  nonlinear  finite  rubber 
viscoelasticity: theoretical aspects and algorithmic treatment for the FE method” 
Computational Mechanics, 44(6), 809-823, (2009). 
DeRuntz, J.A.  Jr., “Reference Material for USA, The Underwater Shock Analysis Code, 
USA-STAGS,  and  USA-STAGS-CFA,”  Report  LMSC-P032568,  Computational 
Mechanics Laboratory, Lockheed Palo Alto Research Laboratory, Palo Alto, CA.  
(1993). 
Desai,  C.S.,  and  H.J.    Siriwardane,  Constitutive  Laws  for  Engineering  Materials  with 
Emphasis On Geologic Materials, Prentice-Hall, Chapter 10, (1984). 
Deshpande, V.S.  and N.A.  Fleck, “Isotropic Models for Metallic Foams,” Journal of the 
Mechanics and Physics of Solids, 48, 1253-1283, (2000).
REFERENCES 
Dick,  R.E.,  and  W.H.    Harris,  “Full  Automated  Rezoning  of  Evolving  Geometry 
Problems,” Numerical Methods in Industrial Forming Processes, Chenot, Wood, 
and Zienkiewicz, Editors, Bulkema, Rotterdam, 243-248, (1992). 
Dilger, W.H., R.  Koch, and R.  Kowalczyk, “Ductility of Plain and Confined Concrete 
Under Different Strain Rates,” ACI Journal, January-February, (1984). 
Dobratz,  B.M.,  “LLNL  Explosives  Handbook,  Properties  of  Chemical  Explosives  and 
Explosive  Simulants,”  University  of  California,  Lawrence  Livermore  National 
Laboratory, Rept.  UCRL-52997 (1981). 
Du  Bois,  P.A.,  “Numerical  Simulation  of  Strandfoam”  Daimler-Chrysler  AG  Abt.  
EP/CSV, Report (2001).   
Dufailly, J., and Lemaitre, J., “Modeling very low cycle fatigue”, International Journal of 
damage mechanics, 4, pp.  153-170 (1995). 
Erhart, T., Andrade, F., Du Bois, P., “Short Introductionof a New Generalized Damage 
Model”, 11th European LS-DYNA Conference, Salzburg, Austria, May 2017. 
Erhart, T., “A New Feature to Model Shell-Like Structures with Stacked Elements”, 10th 
European LS-DYNA Conference, Würzburg, Germany, June 2015. 
Erhart,  T.,  “An  Overview  of  User  Defined  Interfaces  in  LS-DYNA”,  LS-DYNA  Forum, 
Bamberg, Germany, 2010. 
Englemann,  B.    E.,  R.G.    Whirley,  and  G.L.    Goudreau,  “A  Simple  Shell  Element 
Formulation for Large-Scale Elastoplastic Analysis,” CED-Vol.  3. Analytical and 
Computational  Models  of  Shells,  A.K.    Noor,  T.    Belytschko,  and  J.C.    Simo, 
Editors, 1989, pp.  399-416. 
Faßnacht,  W.,  “Simulation  der  Rißbildung  in  Aluminiumgußbauteilen,”    Dissertation, 
Technishe Universität Darmstadt, (1999). 
Feng,  W.W.    and  Hallquist,  J.O.,  “On  Constitutive  Equations  for  Elastomers  and 
Elastomeric  Foams”,  The  4th  European  LS-DYNA  Conference,  D-II-15,  Ulm, 
Germany, May 2003. 
Feucht,  M.,  “Ein  gradientenabhängiges  Gursonmodell  zur  Beshreibung  duktiler 
Schädigung  mit  Entfestigung,”    Dissertation,  Technishe  Universität  Darmstadt, 
(1998). 
Fiolka,  M.    and  Matzenmiller,  A.,  “Delaminationsberechnung  von  Faserverbund-
strukturen”, PAMM Proc. Appl.  Math.  Mech. 5, S.393-394 (2005).
REFERENCES 
Flanagan,  D.P.    and  T.    Belytschko,  “A  Uniform  Strain  Hexahedron  and  Quadrilateral 
and  Orthogonal  Hourglass  Control,”  Int.    J.    Numer.    Meths.    Eng.,  17,  679-706 
(1981). 
Fleischer,  M.,  Borrvall,  T.    and  Bletzinger,  K-U.,  “Experience  from  using  recently 
implemented  enhancements  for  Material  36  in  LS-DYNA  971  performing  a 
virtual tensile test”, 6th European LS-DYNA Users Conference, Gothenburg, 2007. 
Forghani  A.,  “A  Non-Local  Approach  to  Simulation  of  Damage  in  Composite 
Structures”,  PhD  Thesis,  Department  of  Civil  Engineering,  The  University  of  British 
Columbia,, Vancouver, Canada, (2011). 
Forghani A., Zobeiry N., Vaziri R., Poursartip A., and Ellyin F., “A Non-Local Approach 
to  Simulation  of  Damage  in  Laminated  Composites.”  Proc.,  ASC/CANCOM 
Conference, Montreal, Canada (2011b). 
Forghani  A.,  Zobeiry  N.,  Poursartip  A.,  and  Vaziri  R.,  “A  Structural  Modeling 
Framework  for  Prediction  of  Damage  Development  and  Failure  of  Composite 
Laminates”.  Accepted for publication in Composites Sci.  Technol. 
Freed  AD.,  Einstein  DR.    and  Vesely  I.,  “Invariant  Formulation  for  Dispersed 
Transverse  Isotropy  in  Aortic  Heart  Valves  –  An  Efficient  Means  for  Modeling 
Fiber Splay”, Biomechan Model Mechanobiol, 4, 100-117 (2005) 
Fung, Y.C., Biomechanics, Springer, New York, 1993. 
Fung, Y.C., Foundations of Solid Mechanics, Prentice Hall, Inc., Englewood Cliffs, New 
Jersey, 1965. 
Gerlach,  S.,  Fiolka  M.    and  Matzenmiller,  A.,  Modelling  and  analysis  of  adhesively 
bonded joints with interface elements for crash analysis, 4.  LS-DYNA Forum, 20-
21, (2005) Bamberg, DYNAmore GmbH, Stuttgart. 
Ginsberg,  M.    and  J.    Johnson,  “Benchmarking  the  Performance  of  Physical  Impact 
Simulation  Software  on  Vector  and  Parallel  Computers,”  Applications  Track  of 
Supercomputing, IEEE monograph, Computer Society Press, March, 1989. 
Giroux,  E.D.  HEMP  User’s  Manual,  University  of  California,  Lawrence  Livermore 
National Laboratory, Rept.  UCRL-51079 (1973). 
Goldberg, R., and D.  Stouffer, “High Strain Rate Dependent Modeling Polymer Matrix 
Composites,” NASA/TM-1999-209433 (1999). 
Goudreau,  G.L.    and  J.O.    Hallquist,  “Recent  Developments  in  Large  Scale  Finite 
Element  Lagrangian  Hydrocode  Technology,”  J.    Comp.    Meths.    Appl.    Mechs.  
Eng., 30 (1982).
REFERENCES 
Goldak, J., Chakravarti, A., and Bibby, M., “A New Finite Element Model for Welding 
Heat Sources,” Metallurgical Transactions B, vol.  15B, pp.  299-305, June, 1984. 
Govindjee,  S.,  Kay,  J.G.,  and  Simo,  J.C.    [1994],  Anisotropic  Modeling  and  Numerical 
Simulation  of  Brittle  Damage  in  Concrete,  Report  No.    UCB/SEMM-94/18, 
Department of Civil Engineering, University of California, Berkeley, CA 94720. 
Govindjee,  S.,  Kay,  J.G.,  and  Simo,  J.C.    [1995],  “Anisotropic  Modeling  and  Numerical 
Simulation  of  Brittle  Damage  in  Concrete,”  Int.    J.    Numer.    Meth.    Engng,    38, 
3611-3633. 
Graefe,  H.,  W.    Krummheuer,  and  V.    Siejak,  “Computer  Simulation  of  Static 
Deployment Tests for Airbags, Air Permeability of Uncoated Fabrics and Steady 
State  Measurements  of  the  Rate  of  Volume  Flow  Through  Airbags,”  SAE 
Technical  Paper  Series,  901750,  Passenger  Car  Meeting  and  Expositition, 
Dearborn, Michigan, September 17-20, 1990. 
Gran,  J.K.    and  P.E.    Senseny,  “Compression  Bending  of  Scale-Model  Reinforced-
Concrete Walls,” ASCE Journal of Engineering Mechanics, Volume 122, Number 7, 
pages 660-668, July (1996).  
Grassl, P., U.  Nyström, R.  Rempling, and K.  Gylltoft, “A Damage-Plasticity Model for 
the  Dynamic  Failure  of  Concrete”,  8th  International  Conference  on  Structural 
Dynamics, Leuven, Belgium, March (2011). 
Grassl, P., D.  Xenos, U.  Nyström, R.  Rempling, and K.  Gylltoft, “CDPM2: A damage-
plasticity  approach  to  modelling  the  failure  of  concrete”,  International  Journal  of 
Solids and Structures, Vol.  50, Issue 24, pp.  3805-3816, (2013). 
Grassl,  P.    and  M.    Jirásek,  “Damage-Plastic  Model  for  Concrete  Failure”,  International 
Journal  of  Solids  and  Structures,  Vol.    43,  Issues  22-23,  pp.    7166-7196,  November 
(2006). 
Guccione,  J.,  A.    McCulloch,  and  L.    Waldman,  “Passive  Material  Properties  of  Intact 
Ventricular Myocardium Determined from a Cylindrical Model”,  ASME Journal 
of Biomechanical Engineering, Vol.  113, pages 42-55, (1991). 
Guccione  JM,  Waldman  LK,  McCulloch  AD.,  “Mechanics  of  Active  Contraction  in 
Cardiac Muscle: Part II – Cylindrical Models of the Systolic Left Ventricle”, J.  Bio 
Mech, 115, 82-90, (1993). 
Gurson,  A.L.,  Plastic  Flow  and  Fracture  Behavior  of  Ductile  Materials  Incorporating 
Void  Nucleation,  Growth,  and  Interaction,  Ph.D.    Thesis,  Brown  University, 
(1975).
REFERENCES 
Gurson, A.L., “Continuum Theory of Ductile Rupture by Void Nucleation and Growth: 
Part  I  -  Yield  Criteria  and  Flow  Rules  for  Porous  Ductile  Media”,  J.    of  Eng.  
Materials and Technology, (1977). 
Hallquist,  J.O.,  Preliminary  User’s  Manuals  for  DYNA3D  and  DYNAP  (Nonlinear 
Dynamic  Analysis  of  Solids  in  Three  Dimension),  University  of  California, 
Lawrence Livermore National Laboratory, Rept.  UCID-17268 (1976) and Rev.  1 
(1979).[a] 
Hallquist,  J.O.,  A  Procedure  for  the  Solution  of  Finite  Deformation  Contact-Impact 
Problems  by  the  Finite  Element  Method,  University  of  California,  Lawrence 
Livermore National Laboratory, Rept.  UCRL-52066 (1976). 
Hallquist,  J.O.,  “A  Numerical  Procedure  for  Three-Dimensional  Impact  Problems,” 
American Society of Civil Engineering, Preprint 2956 (1977). 
Hallquist,  J.O.,  “A  Numerical  Treatment  of  Sliding  Interfaces  and  Impact,”  in:  K.C.  
Park  and  D.K.    Gartling  (eds.)  Computational  Techniques  for  Interface  Problems, 
AMD Vol.  30, ASME, New York (1978). 
Hallquist, J.O., NIKE2D: An Implicit, Finite-Element Code for Analyzing the Static and 
Dynamic  Response  of  Two-Dimensional  Solids,  University  of  California, 
Lawrence Livermore National Laboratory, Rept.  UCRL-52678 (1979).[b] 
Hallquist,  J.O.,  User's  Manual  for  DYNA2D  –  An  Explicit  Two-Dimensional 
Hydrodynamic  Finite  Element  Code  with  Interactive  Rezoning,  University  of 
California, Lawrence Livermore National Laboratory, Rept.  UCID-18756 (1980). 
Hallquist, J.O., User's Manual for DYNA3D and DYNAP (Nonlinear Dynamic Analysis 
of  Solids  in  Three  Dimensions),  University  of  California,  Lawrence  Livermore 
National Laboratory, Rept.  UCID-19156 (1981).[a] 
Hallquist,  J.    O.,  NIKE3D:  An  Implicit,  Finite-Deformation,  Finite-Element  Code  for 
Analyzing  the  Static  and  Dynamic  Response  of  Three-Dimensional  Solids, 
University of California, Lawrence Livermore National Laboratory, Rept.  UCID-
18822 (1981).[b] 
Hallquist,  J.O.,  DYNA3D  User's  Manual  (Nonlinear  Dynamic  Analysis  of  Solids  in 
Three  Dimensions),  University  of  California,  Lawrence  Livermore  National 
Laboratory, Rept.  UCID-19156 (1982; Rev.  1: 1984; Rev.  2: 1986). 
Hallquist,  J.O.,  Theoretical  Manual  for  DYNA3D,  University  of  California,  Lawrence 
Livermore National Laboratory, Rept.  UCID-19501 (March, 1983). 
Hallquist,  J.O.,  DYNA3D  User's  Manual  (Nonlinear  Dynamic  Analysis  of  Solids  in 
Three  Dimensions),  University  of  California,  Lawrence  Livermore  National 
Laboratory, Rept.  UCID-19156 (1988, Rev.  4).
REFERENCES 
Hallquist,  J.O.,  LS-DYNA  User's  Manual  (Nonlinear  Dynamic  Analysis  of  Solids  in 
Three  Dimensions),  Livermore  Software  Technology  Corporation,  Rept.    1007 
(1990). 
Hallquist,  J.O.,  D.J.    Benson,  and  G.L.    Goudreau,  “Implementation  of  a  Modified 
Hughes-Liu  Shell  into  a  Fully  Vectorized  Explicit  Finite  Element  Code,” 
Proceedings  of  the  International  Symposium  on  Finite  Element  Methods  for 
Nonlinear Problems, University of Trondheim, Trondheim, Norway (1985). 
Hallquist,  J.O.    and  D.J.    Benson,  “A  Comparison  of  an  Implicit  and  Explicit 
Implementation of the Hughes-Liu Shell,” Finite Element Methods for Plate and 
Shell Structures, T.J.R.  Hughes and E.  Hinton, Editors, 394-431, Pineridge Press 
Int., Swanea, U.K.  (1986). 
Hallquist, J.O.  and D.J.  Benson, DYNA3D User’s Manual (Nonlinear Dynamic Analysis 
of  Solids  in  Three  Dimensions),  University  of  California,  Lawrence  Livermore 
National Laboratory, Rept.  UCID-19156 (Rev.  2: 1986; Rev.  3: 1987). 
Hallquist,  J.O.,  D.W.    Stillman,  T.J.R.    Hughes,  C.    and  Tarver,”Modeling  of  Airbags 
Using MVMA/DYNA3D,” LSTC Report (1990). 
Hashin,  Z,  “Failure  Criteria  for  Unidirectional  Fiber  Composites,”  Journal  of  Applied 
Mechanics, 47, 329 (1980). 
Haßler,  M.,  Schweizerhof,  K.,  “On  the  influence  of  fluid-structure-interaction  on  the 
static  stability  of  thin  walled  shell  structures”,  International  Journal  of  Structural 
Stability, Vol.  7, pp.  313–335, (2007). 
Haßler,  M.,  Schweizerhof,  K.,  “On the  static  interaction of  fluid  and  gas  loaded  multi-
chamber  systems  in  a  large  deformation  finite  element  analysis”,  Computer 
Methods in Applied Mechanics and Engineering, Vol.  197, pp.  1725–1749, (2008). 
Hänsel,  C.,  P.    Hora,  and  J.    Reissner,  “Model  for  the  Kinetics  of  Strain-Induced 
Martensitic Phase Transformation at Isothermal Conditions for the Simulation of 
Sheet Metal Forming Processes with Metastable Austenitic Steels,” Simulation of 
Materials Processing: Theory, Methods, and Applications, Huétink and Baaijens 
(eds), Balkema, Rotterdam, (1998). 
Haward,  R.N.,  and  Thackray,  G.,  “The  use  of  a  mathematical  model  to  describe 
isothermal  stress-strain  curves  in  glassy  thermoplastics”.  Proc  Roy  Soc  A,  302, 
453-472 (1968). 
Herrmann,  L.R.    and  F.E.    Peterson,  “A  Numerical  Procedure  for  Viscoelastic  Stress 
Analysis,”  Seventh  Meeting  of  ICRPG  Mechanical  Behavior  Working  Group, 
Orlando, FL, CPIA Publication No.  177, 1968.
REFERENCES 
Hill A.V., “The heat of shortening and the dynamic constants of muscle,” Proc Roy Soc 
B126:136-195, (1938). 
Hill, R., “A Theory of the Yielding and Plastic Flow of Anisotropic Metals,” Proceedings 
of the Royal Society of London, Series A., Vol.  193, pp.  281-197 (1948). 
Hill, R., “Aspects of Invariance in Solid Mechanics,” Advances in Applied Mechanics, Vol.  
18, pp.  1-75 (1979). 
Hill,  R.,  “Constitutive  Modeling  of  Orthotropic  Plasticity  in  Sheet  Metals,”  J.    Mech.  
Phys.  Solids, Vol.  38, No.  3, 1989, pp.  405-417. 
Hippchen, P., Merklein, M., Lipp, A., Fleischer, M., Grass, H., Craighero, P., “Modelling 
kinetics  of  phase  transformation  for  the  indirect  hot  stamping  process”,  Key 
Engineering Materials, Vol.  549, pages 108-116, (2013). 
Hippchen,  P.,  “Simulative  Prognose  der  Geometrie 
indirekt  pressgehärteter 
Karosseriebauteile  für  die  industrielle  Anwendung”,  Dissertation,  Technische 
Fakultät  der  Friedrich-Alexander  Universität  Erlangen-Nürnberg,  Meisenbach 
Verlag Bamberg, Band 249, (2014). 
Hirth, A., P.  Du Bois, and K.  Weimar, “Improvement of LS-DYNA Material Law 83 (Fu 
Chang)  for  the  Industrial  Simulation  of  Reversible  Energy-Absorbing  Foams,” 
CAD-FEM  User's  Meeting,  Bad  Neuenahr  -  Ahrweiler,  Germany,  October  7-9, 
Paper 2-40, (1998). 
Hollenstein  M.,  M.    Jabareen,  and  M.B.    Rubin,  “Modelling  a  smooth  elastic-inelastic 
transition  with  a  strongly  objective  numerical  integrator  needing  no  iteration”, 
Comput.  Mech., Vol.  52, pp.  649-667, DOI 10.1007/s00466-013-0838-7 (2013). 
Hollenstein M., M.  Jabareen, and M.B.  Rubin, “Erratum to: Modelling a smooth elastic-
inelastic  transition  with  a  strongly  objective  numerical  integrator  needing  no 
iteration”, Comput.  Mech., DOI 10.1007/s00466-014-1099-9 (2014). 
Holmquist, T.J., G.R.  Johnson, and W.H.  Cook, “A Computational Constitutive Model 
for Concrete Subjected to Large Strains, High Strain Rates, and High Pressures”, 
Proceedings  14th  International  Symposium  on  Ballistics,  Quebec,  Canada,  pp.  
591-600, (1993). 
Hopperstad, O.S.  and Remseth, S.,” A return Mapping Algorithm for a Class of Cyclic 
Plasticity Models”, International Journal for Numerical Methods in Engineering, Vol.  
38, pp.  549-564, (1995). 
Huang, Yuli, private communication, Livermore, (2006). 
Hughes,  T.J.R.    and  E.    Carnoy,  “Nonlinear  Finite  Element  Shell  Formulation 
Accounting for Large Membrane strains,” AMD-Vol.48, ASME, 193-208 (1981).
REFERENCES 
Hughes,  T.J.R.    and  W.K.    Liu,  “Nonlinear  Finite  Element  Analysis  of  Shells:  Part  I.  
Three-Dimensional Shells.” Comp.  Meths.  Appl.  Mechs., 27, 331-362 (1981a). 
Hughes,  T.J.R.    and  W.K.    Liu,  “Nonlinear  Finite  Element  Analysis  of  Shells:  Part  II.  
Two-Dimensional Shells.” Comp.  Meths.  Appl.  Mechs., 27, 167-181 (1981b). 
Hughes, T.J.R., W.K.  Liu, and I.  Levit, “Nonlinear Dynamics Finite Element Analysis of 
  W.  
Shells.”  Nonlinear  Finite  Element  Analysis  in  Struct. 
Wunderlich, E.  Stein, and K.J.  Bathe, Springer-Verlag, Berlin, 151- 168 (1981c).  
  Mech.,  Eds. 
Huh,  H.,  Chung,  K.,  Han,  S.S.,  and  Chung,  W.J.,  “The  NUMISHEET  2011  Benchmark 
Study  of  the  8th  International  Conference  and  Workshop  on  Numerical 
Simulation  of  3D  Sheet  Metal  Forming  Processes,  Part  C  Benchmark  Problems 
and Results”, p 171-228, Seoul, Korea, August, 2011. 
Huh,  H.    and  Kang,  W.J.,  “Crash-Worthiness  Assessment  of  Thin-Walled  Structures 
with the High-Strength Steel Sheet”, Int.  Journal of Vehicle Design, Vol.  30, Nos.  
1/2 (2002). 
Ibrahimbegovic,  A.    and  Wilson,  E.L.    “A  unified  formulation  for  triangular  and 
quadrilateral flat shell finite elements with six nodal degrees of freedom”, Comm.  
Applied Num.  Meth, 7, 1-9 (1991). 
Isenberg,  J.,  Vaughan,  D.K.,  Sandler,  I.S.,  Nonlinear  Soil-Structure  Interaction,  Electric 
Power Research Institute report EPRI NP-945, Weidlinger Associates (1978). 
Ivanov,  I.,  and  A.    Tabiei,  “Loosely  Woven  Fabric  Model  With  Viscoelastic  Crimped 
Fibers for Ballistic Impact Simulations”, IJNME, 57, (2004). 
Jabareen,  M.,  “Strongly  objective  numerical  implementation  and  generalization  of  a 
unified  large  inelastic  deformation  model  with  a  smooth  elastic-inelastic 
transition”, submitted to Int.  J.  Solids and Struct.  (2015). 
Jabareen,  M.,  and  Rubin,  M.B.,  A  Generalized  Cosserat  Point  Element  (CPE)  for 
Isotropic  Nonlinear  Elastic  Materials  including  Irregular  3-D  Brick  and  Thin 
Structures, J.  Mech.  Mat.  And Struct., Vol 3-8, 1465-1498 (2008). 
Jabareen,  M.,  Hanukah,  E.    and  Rubin,  M.B.,  A  Ten  Node  Tetrahedral  Cosserat  Point 
Element (CPE) for Nonlinear Isotropic Elastic Materials, J.  Comput.  Mech.  52, 
257-285 (2013). 
Johnson,  G.C.    and  D.J.    Bammann,  “A  discussion  of  stress  rates  in  finite  deformation 
problems,” Int.  J.  Solids Struct, 20, 725-737 (1984). 
Johnson, G.R.  and W.H.  Cook, “A Constitutive Model and Data for Metals Subjected to 
Large  Strains,  High  Strain  Rates  and  High  Temperatures.”    Presented  at  the
REFERENCES 
Seventh  International  Symposium  on  Ballistics,  The  Hague,  The  Netherlands, 
April 1983. 
Johnson,  G.R.    and  T.J.    Holmquist,  “An  Improved  Computational  Model  for  Brittle 
Materials” in High-Pressure Science and Technology - 1993 American Institute of 
Physics Conference Proceedings 309 (c 1994) pp.981-984  ISBN 1-56396-219-5. 
Jones,  R.M.,  Mechanics  of  Composite  Materials,  Hemisphere  Publishing  Corporation, 
New York, (1975). 
Kenchington, G.J., “A Non-Linear Elastic Material Model for DYNA3D,” Proceedings of 
the DYNA3D Users Group Conference, published by Boeing Computer Services 
(Europe) Limited (1988). 
Key,  S.W.  HONDO  – A  Finite  Element  Computer  Program for  the  Large  Deformation 
Dynamic  Response  of  Axisymmetric  Solids,  Sandia  National  Laboratories, 
Albuquerque, N.M., Rept.  74-0039 (1974). 
Kolling,  S.,  Haufe,  A.,  Feucht,  M.,  DuBois,  P.    A.    “SAMP-1:  A  Semi-Analytical  Model 
for  the  Simulation  of  Polymers”,  4.    LS-DYNA  Anwenderforum,  October  20-21, 
Bamberg, Germany, (2005). 
Kolling,  S.,  Hirth,  A.,  Erhart,  and  Du  Bois  P.A.,  Private  Communication,  Livermore, 
California (2006).   
Krieg,  R.D.,A  Simple  Constitutive  Description  for  Cellular  Concrete,  Sandia  National 
Laboratories, Albuquerque, NM, Rept.  SC-DR-72-0883 (1972). 
Krieg,  R.D.    and  S.W.    Key,  “Implementation  of  a  Time  Dependent  Plasticity  Theory 
into  Structural  Computer  Programs,”  Vol.    20  of  Constitutive  Equations  in 
Viscoplasticity:  Computational  and  Engineering  Aspects  (American  Society  of 
Mechanical Engineers, New York, N.Y.,  pp.  125-137 (1976). 
Lademo, O.G., Berstad, T., Tryland, T., Furu, T., Hopperstad, O.S.  and Langseth, M., “A 
model  for  process-based  crash  simulation”,  8th  International  LS-DYNA  User’s 
Conference, Detroit, May 3-5, 2004.    
Lademo,  O.G.,  Hopperstad,  O.S.,  Berstad,  T.    and  Langseth  M.,  “Prediction  of  Plastic 
Instability  in  Extruded  Aluminum  Alloys  Using  Shell  Analysis  and  a  Coupled 
Model  of  Elasto-plasticity  and  Damage,”  Journal  of  Materials  Processing 
Technology, 2002 (Article in Press).     
Lademo, O.G., Hopperstad, O.S., Malo, K.A.  and Pedersen, K.O., “Modelling of Plastic 
Anisotropy  in  Heat-Treated  Aluminum  Extrusions”,  Journal  of  Materials 
Processing Technology 125-126, pp.  84-88 (2002).
REFERENCES 
Lee,  E.L.    and  C.M.    Tarver,  “Phenomenological  Model  of  Shock  Initiation  in 
Heterogenous Explosives,” PHYS.  Fluids, Vol.  23, p.  2362 (1980). 
Lee,  Y.    L.    and  S  Balur  of  Chrysler  Group  LLC,  “Method  of  predicting  spot  weld 
failure”  (Attorney  Docket  No  708494US2),  filed  on  December  22,  2011  and 
assigned US Serial No.  13/334,701. 
Lemaitre, J., A Course on Damage Mechanics, Springer-Verlag, (1992). 
Lemaitre,  J.,  and  Chaboche,  J.L.,  Mechanics  of  Solid  Materials,  Cambridge  University 
Press,        (1990). 
Lemmen,  P.    P.    M.    and  Meijer,  G.    J.,  “Failure  Prediction  Tool  Theory  and  User 
Manual,” TNO Report 2000-CMC-R0018, (2001).  
Lewis,  B.A.,  “Developing  and  Implementing  a  Road  Side  Safety  Soil  Model  into  LS-
DYNA,” FHWA Research and Development Turner-Fairbank Highway Research 
Center, (1999). 
Li, Y.H.  and Sellars, C.M., “Modeling Deformation Behavior of Oxide Scales and their 
Effects on Interfacial Heat Transfer and Friction during Hot Steel Rolling”, Proc.  
Of  the  2nd  Int.    Conf.    Modeling  of  Metals  Rolling  Processes,  The  Insitute  of 
Materials, Londong, UK, 192-201 (1996).   
Lindström P.R.M, “DNV Platform of Computational Welding Mechanics”, Proc.  of Int.  
Inst.  Welding 66th Annual Assembly (2013).  
Lindström,  P.,  "Improved  CWM  platform  for  modelling  welding  procedures  and  their 
effects on structural behaviour", PhD Thesis, Production Technology, University 
West, Trollhättan, Sweden (2015). 
Lian, W., personal communication: “LS-DYNA Airbag Module Improvement Request”, 
General Motors Corporation (2000). 
Y.  Luo, “An Efficient 3D Timoshenko Beam Element with Consistent Shape Functions” 
Adv.  Theor.  Appl.  Mech., 1(3), 95-106, (2008).  
MADYMO3D  USER’S  MANUAL,  Version  4.3,  TNO  Road-Vehicles  Research  Institute, 
Department of Injury Prevention, The Hague, The Netherlands, (1990). 
Maimí, P., Camanho, P.P., Mayugo, J.A., Dávila, C.G., “A continuum damage model for 
composite laminates: Part I – Constitutive model”, Mechanics of Materials, Vol.  39, 
pp.  897–908, (2007). 
Maimí, P., Camanho, P.P., Mayugo, J.A., Dávila, C.G., “A continuum damage model for 
composite  laminates:  Part  II  –  Computational  implementation  and  validation”, 
Mechanics of Materials, Vol.  39, pp.  909–919, (2007).
REFERENCES 
Maker,  B.N.,  Private  communication  Lawrence  Livermore  National  Laboratory,  Dr.  
Maker  programmed  and  implemented  the  compressible  Mooney  Rivlin  rubber 
model (1987).  
Makris  N.    and  Zhang,  J.,  “Time-domain  visco-elastic  analysis  of  earth  structures,” 
Earthquake Engineering and Structural Dynamics, vol.  29, pp.  745–768, (2000). 
Malvar, L.J., Crawford, J.E., Morrill, K.B., K&C Concrete Material Model Release III —
Automated  Generation  of  Material  Model  Input,  K&C  Technical  Report  TR-99-
24-B1, 18 August 2000 (Limited Distribution). 
Malvar, L.J., Crawford, J.E., Wesevich, J.W., Simons, D., “A Plasticity Concrete Material 
Model  for  DYNA3D,”  International  Journal  of  Impact  Engineering,  Volume  19, 
Numbers 9/10,  pages 847-873, December 1997. 
Malvar,  L.J.,  and  Ross,  C.A.,  “Review  of Static  and  Dynamic  Properties  of  Concrete  in 
Tension,”  ACI  Materials  Journal,  Volume  95,  Number  6,  pages  735-739, 
November-December 1998. 
Malvar,  L.J.,  and  Simons,D.,  “Concrete  Material  Modeling  in  Explicit  Computations,” 
Proceedings,  Workshop  on  Recent  Advances  in  Computational  Structural 
Dynamics  and  High  Performance  Computing,  USAE  Waterways  Experiment 
Station,  Vicksburg,  MS,  pages  165-194,  April  1996.    (LSTC  may  provide  this 
reference upon request.) 
Malvar,  H.S.,  Sullivan,  G.S.,  and  Wornell,  G.W.,  “Lapped  Orthogonal  Vector 
Quantization”, in Proc.  Data Compression Conference, Snowbird, Utah, 1996. 
Marin, E.B., unpublished paper, Sandia National Laboratory, CA (2005).  
Matzenmiller,  A. 
  and  Burbulla,  F.,  “  Robustheit  und  Zuverlässigkeit  der 
Berechnungsmethoden  von  Klebverbindungen  mit  hochfesten  Stahlblechen 
unter Crashbedingungen” (2013), http://www.ifm.maschinenbau.uni-kassel.de/
~amat/publikationen/p75_p828-modellerweiterung.pdf 
Matzenmiller, A., Lubliner, J., and Taylor, R.L., “A Constitutive Model for Anisotropic 
Damage  in  Fiber-Composites,”  Mechanics  of  Materials,  Vol.    20,  pp.    125-152 
(1995). 
Matzenmiller,  A.    and  J.    K.    Schweizerhof,  “Crashworthiness  Considerations  of 
Composite Structures – A First Step with Explicit Time Integration in Nonlinear 
Computational  Mechanics–State-of-the-Art,”  Ed.    P.    Wriggers,  W.    Wagner, 
Springer Verlay, (1991). 
Mauldin, P.J., R.F.  Davidson, and R.J.  Henninger, “Implementation and Assessment of 
the Mechanical-Threshold-Stress Model Using the EPIC2 and PINON Computer 
Codes,”  Report LA-11895-MS, Los Alamos National Laboratory (1990).
REFERENCES 
Maurer,  A.,  Gebhardt,  M.,  Schweizerhof,  K.,  “Computation  of  fluid  and/or  gas  filled 
inflatable dams“, LS-Dyna Forum, Bamberg, Germany, (2010). 
McCormick,  P.G.,  “Theory  of  flow  localization  due  to  dynamic  strain  ageing,”  Acta 
Metallurgica, 36, 3061-3067 (1988). 
Mi Y., Crisfield, M.A., Davies, A.O.  Progressive delamination using interface elements. 
J Compos Mater, 32(14)1246-72 (1998). 
Moran, B., Ortiz, M.  and Shih, C.F., “Formulation of implicit finite element methods for 
multiplicative finite deformation plasticity”. Int J for Num Methods in Engineering, 
29, 483-514 (1990). 
de  Moura  MFSF,  Gonçalves,  J.P.,  Marques,  A.T.,  and  de  Castro,  P.T.,  Elemento  finito 
isoparamétrico de interface para problemas tridimensionais. Revista Internacional 
de Métodos Numéricos Para Cálculo e Diseño en Ingeniería, 14:447-66 (1996). 
Murray,  Y.D.,  Users  Manual  for  Transversely  Isotropic  Wood  Model  APTEK,  Inc., 
Technical Report to the FHWA (to be published) (2002). 
Murray,  Y.D.   and  Lewis,  B.A.,  Numerical  Simulation  of  Damage  in  Concrete  APTEK, 
Inc.,  Technical  Report  DNA-TR-94-190,  Contract  DNA  001-91-C-0075,  Defense 
Nuclear Agency, Alexandria VA 22310. 
Murray,  Y.D.,  Users  Manual  for  LS-DYNA  Concrete  Material  Model  159,  Report  No.  
FHWA-HRT-05-062, Federal Highway Administration, (2007).  
Murray, Y.D., A.  Abu-Odeh, and R.  Bligh, Evaluation of Concrete Material Model 159, 
Report No.  FHWA-HRT-05-063, Federal Highway Administration, (2007). 
Muscolini,  G.,  Palmeri,  A.    and  Ricciardelli,  F.,  “Time-domain  response  of  linear 
hysteretic  systems  to  deterministic  and  random  excitations,”  Earthquake 
Engineering and Stuctrual Dynamics, vol.  34, pp.  1129–1147, (2005). 
Nagararaiah,  Reinhorn,  &  Constantinou,  “Nonlinear  Dynamic  Analysis  of  3-D  Base-
Isolated Structures”, Jounal of Structural Engineering Vol 117, No 7, (1991). 
Nahshon,  K.    and  Hutchinson,  J.W.,  “Modification  of  the  Gurson  Model  for  shear 
failure”, European Journal of Mechanics A/Solids, Vol.  27, 1-17, (2008). 
Naik  D.,  Sankaran  S.,  Mobasher  D.,  Rajan  S.D.,  Pereira  J.M.,  “Development  of  reliable 
modeling  methodologies  for  fan  blade  out  containment  analysis  –  Part  I: 
Experimental studies”, International Journal of Impact Engineering, Volume 36, 
Issue 1, Pages 1-11, (2009) 
Neal, M.O., C-H Lin, and J.  T.  Wang, “Aliasing Effects on Nodal Acceleration Output 
International 
from  Nonlinear  Finite  Element  Simulations,”  ASME  2000
REFERENCES 
Mechanical  Engineering  Congress  and  Exposition,  Orlando,  Florida,  November 
5-10, (2000). 
Neilsen, M.K., H.S.  Morgan, and R.D.  Krieg, “A Phenomenological Constitutive Model 
for  Low  Density  Polyurethane  Foams,”  Rept.    SAND86-2927,  Sandia  National 
Laboratories, Albuquerque, N.M., (1987). 
Nusholtz,  G.,  W.    Fong,  and  J.    Wu,  “Air  Bag  Wind  Blast  Phenomena  Evaluation,” 
Experimental Techniques, Nov.-Dec.  (1991). 
Nusholtz,  G.,  D.    Wang,  and  E.B.    Wylie,  “Air  Bag  Momentum  Force  Including 
Aspiration,” Preprint, Chrysler Corporation, (1996). 
Nusholz, private communication, (1996). 
Nygards, M., M.  Just, and J.  Tryding, “Experimental and numerical studies of creasing 
of paperboard,” Int.  J.  Solids and Struct., 46, 2493-2505 (2009). 
Ogden,  R.W.,  Non-Linear  Elastic  Deformations,  Ellis  Horwood  Ltd.,  Chichester,  Great 
Britian (1984). 
Oliver,  J.,  “A  Consistent  Characteristic  Length  of  Smeared  Cracking  Models,” 
International Journal for Numerical Methods in Engineering, 28, 461-474 (1989). 
Papadrakakis, M., “A Method for the Automatic Evaluation of the Dynamic Relaxation 
Parameters,” Comp.  Meth.  Appl.  Mech.  Eng., Vol.  25, pp.  35-48 (1981). 
Park, R.  and Paulay, T., (1975) Reinforced Concrete Structures, J.  Wiley and Sons, New 
York.  
Park, Y.J., Wen, Y.K, and Ang, A.H-S, “Random Vibration of Hysteretic Systems Under 
Bi-directional Ground  Motions”, Earthquake  Engineering and Structural Dynamics, 
Vol.  14, pp.  543-557 (1986). 
Penelis, G.G.  and Kappos, A.J., Earthquake-Resistant Concrete Structures, E&FN Spon., 
(1997). 
Pijaudier-Cabot, G., and Bazant, Z.P., “Nonlocal Damage Theory,” Journal of Engineering 
Mechanics, ASCE, Vol.  113, No.  10, 1512-1533 (1987). 
Pinho, S.T., Iannucci, L., Robinson, R., “Physically-based failure models and criteria for 
laminated  fibre-reinforced  composites  with  emphasis  on  fibre  kinking:  Part  I: 
Development”, Composties Part A, Vol.  37, 63-73 (2006). 
Pinho, S.T., Iannucci, L., Robinson, R., “Physically-based failure models and criteria for 
laminated fibre-reinforced composites with emphasis on fibre kinking: Part II: FE 
implementation”, Composties Part A, Vol.  37, 766-777 (2006).
REFERENCES 
Porcaro,  R.,  A.G.    Hanssen,  A.    Aalberg  and  M.    Langseth,  “The  behaviour  of  aself-
piercing riveted connection under quasi-static loading conditions,” Int.  J.  Solids 
and Structures, Vol.  43/17, pp.  5110-5131 (2006). 
Porcaro,  R.,  A.G.    Hanssen,  A.    Aalberg  and  M.    Langseth,  “Self-piercing  riveting 
process,  an  experimental  and  numerical  investigation,”  Journal  of  Materials 
processing Technology, Vol.  171/1, pp.  10-20 (2006). 
Porcaro,  R.,  M.    Langseth,  A.G.    Hanssen,  H.    Zhao,  S.    Weyer  and  H.    Hooputra, 
“Crashworthiness  of  self-piercing  riveted  connections,”  International  Journal  of 
Impact Engineering, In press, Accepted manuscript (2007). 
Puck,  A.,  Kopp,  J.,  Knops,  M.,  “Guidelines  for  the  determination  of  the  parameters  in 
Puck’s  action  plane  strength  criterion”,  Composites  Science  and  Technology,  Vol.  
62, 371-378 (2002). 
Puso,  M.A.,  “A  Highly  Efficient  Enhanced  Assumed  Strain  Physically  Stabilized 
Hexahedral Element”, Int.  J.  Numer.  Meth.  Eng., Vol.  49, 1029-1064 (2000). 
Puso, M.A., and Laursen, T.A., “A Mortar segment-to-segment contact method for large 
deformation solid mechanics”, Comput.  Methods Appl.  Mech.  Engrg.  193 (2004) 601-
629. 
Puso, M.A., and Laursen, T.A., “A Mortar segment-to-segment frictional contact 
method for large deformations”, Comput.  Methods Appl.  Mech.  Engrg.  193 (2004) 
4891-4913. 
Puso, M.A.  and Weiss, J.A., “Finite Element Implementation of Anisotropic Quasilinear 
Viscoelasticity  Using  a  Discrete  Spectrum  Approximation”,  ASME  J.    Biomech.  
Engng., 120, 62-70 (1998). 
Pelessone,  D.,  Private  communication,  GA  Technologies,  P.O.    Box  85608,  San  Diego, 
CA., Telephone No.  619-455-2501 (1986). 
Quapp, K.M.  and Weiss, J.A., “Material Characterization of Human Medial Collateral 
Ligament”, ASME J.  Biomech Engng., 120, 757-763 (1998). 
Reyes,  A.,  O.S.    Hopperstad,  T.    Berstad,  and  M.    Langseth,  Implementation  of  a 
Material  Model  for  Aluminium  Foam  in  LS-DYNA,  Report  R-01-02,  Restricted, 
Department  of  Structural  Engineering,  Norwegian  University  of  Science  and 
Technology, (2002). 
Randers-Pehrson, G.  and K.  A.  Bannister, Airblast Loading Model for DYNA2D and 
DYNA3D,  Army  Research  Laboratory,  Rept.    ARL-TR-1310,  publicly  released 
with unlimited distribution, (1997).
REFERENCES 
Richards,  G.T.,  Derivation  of  a  Generalized  Von  Neuman  Psuedo-Viscosity  with 
Directional  Properties,  University  of  California,  Lawrence  Livermore  National 
Laboratory, Rept.  UCRL-14244 (1965). 
Riedel  W.,  Thoma  K.,  Hiermaier  S.    and  Schmolinske  E.,  “Penetration  of  reinforced 
concrete by BETA-B-500”, in Proc.  9. ISIEMS, Berlin Strausberg, Mai (1999).  
Riedel  W.,  “Beton  unter  Dynamischen  Lasten  –    Meso-  und  Makromechanische 
Modelle” In: Ernst-Mach-Institut, editor. Freiburg: Fraunhofer IRB, ISBN 3-8167-
6340-5; 2004.  
Ritto-Corrêa  M.    and  Camotim  D.,  “On  the  arc-length  and  other  quadratic  control 
methods:  Established,  less  known  and  new  implementation  procedures”, 
Comput.  Struct., 86, pp.  1353-1368 (2008). 
Roussis,  P.C.,  and  Constantinou,  M.C.,  “Uplift-restraining  Friction  Pendulum  seismic 
isolation system”, Earthquake Engineering and Structural Dynamics, 35 (5), 577-593, 
(2006).   
Rumpel,  T.,  Schweizerhof,  K.,  “Volume-dependent  pressure  loading  and  its  influence 
on  the  stability  of  structures“,  International  Journal  for  Numerical  Methods  in 
Engineering, Vol.  56, pp. 211-238, (2003). 
Rumpel,  T.,  Schweizerhof,  K.,  “Hydrostatic  fluid  loading  in  non-linear  finite  element 
analysis“, International  Journal  for  Numerical Methods  in  Engineering,  Vol.    59,  pp.  
849–870, (2004). 
Rupp, A., Grubisic, V., and Buxbaum, O., Ermittlung ertragbarer Beanspruchungen am 
Schweisspunkt  auf  Basis  der  ubertragbaren  Schnittgrossen,  FAT  Schriftenreihe 
111, Frankfurt (1994). 
Sala, M.O.  Neal, and J.T.  Wang, Private Communication, General Motors, May, 2004. 
Sackett,  S.J.,  “Geological/Concrete  Model  Development,”  Private  Communication 
(1987). 
Sandler,  I.S.    and  D.    Rubin,  “An  Algorithm  and  a  Modular  Subroutine  for  the  Cap 
Model,” Int.  J.  Numer.  Analy.  Meth.  Geomech., 3, pp.  173-186 (1979). 
Schedin, E., Prentzas, L.  and Hilding D., “Finite Element Simulation of the TRIP-effect 
in Austenitic Stainless Steel,” presented at SAE 2004, SAE Technical paper 2004-
01-0885, (2004).  
Schulte-Frankenfeld N., Deiters, T., “General Introduction to FATXML – data format“, 
https://www.vda.de/dam/vda/publications/FATXML-
Format%20Version%20V1.1/1305643077_de_2066216985.zip, (2016).
REFERENCES 
Schweizerhof,  K.    and  E.    Ramm,  “Displacement  Dependent  Pressure  Loads  in 
Nonlinear Finite Element Analyses,” Comput.  Struct., 18, pp.  1099-1114 (1984). 
Schwer,  L.E.,  “A  Viscoplastic  Augmentation  of  the  Smooth  Cap  Model,”  Nuclear 
Engineering and Design, Vol.  150, pp.  215-223, (1994). 
Schwer,  L.E.,  “Demonstration  of  the  Continuous  Surface  Cap  Model  with  Damage: 
Concrete  Unconfined  Compression  Test  Calibration,”  LS-DYNA  Geomaterial 
Modeling Short Course Notes, July (2001). 
Schwer, L.E., W.  Cheva, and J.O.  Hallquist, “A Simple Viscoelastic Model for Energy 
Absorbers Used in Vehicle-Barrier Impact,” in Computation Aspects of Contact, 
Impact,  and  Penetration,  Edited  by  R.F.    Kulak  and  L.E.    Schwer,  Elmepress 
International, Lausanne, Switzerland, pp.  99-117 (1991). 
Schwer,  L.E.    and  Y.D.    Murray,  “A  Three-Invariant  Smooth  Cap  Model  with  Mixed 
in 
for  Numerical  and  Analytical  Methods 
Hardening,”  International  Journal 
Geomechanics, Volume 18, pp.  657-688, (1994). 
Seeger,  F.,  M.    Feucht,  T.    Frank  (DaimlerChrysler  AG),  and  A.    Haufe,  B.    Keding 
(DYNAmore  GmbH),  “An  Investigation  on  Spotweld  Modeling  for  Crash 
Simulation  with  LS-DYNA”,  4th  LS-DYNA-Forum,  Bamburg,  Germany,  October 
(2005), ISBN 3-9809901-1-7. 
Shi,  M.F.,  and  Gelisse,  S.,  “Issues  on  the  AHSS  Forming  Limit  Determination”, 
International  Deep  Drawing  Research  Group  (IDDRG),  Porto,  Portugal,  June, 
2006. 
Shi,  M.F.,  Zhu,  X.H.,  Xia,  C.,  and  Stoughton  T.,  “Determination  of  Nonlinear 
Isotropic/Kinematic Hardening Constitutive Parameter for AHSS using Tension 
and  Compression  Tests”,    p.    137-142,  Proceedings  of  the  7th  International 
Conference and Workshop on Numerical Simulation of 3D Sheet Metal Forming 
Processes (NUMISHEET 2008), Interlaken, Switzerland, September, 2008. 
Sheppard,  S.D.,  Estimations  of  Fatigue  Propagation  Life  in  Resistance  Spot  Welds, 
ASTM STP 1211, pp.  169-185, (1993). 
Sheppard,  T.    and  Wright,  D.S.,  “Determination  of  flow  stress:  Part  1  constitutive 
equation  for  aluminum  alloys  at  elevated  temperatures”,  Metals  Technology,  p.  
215, June 1979.  
Shvets, I.T.  and Dyban, E., P., “Contact Heat Transfer between Plane Metal Surfaces”, 
Int.  Chem.  Eng., Vol.  4, No.  4, 621 (1964).  
Simo,  J.C.,  J.W.    Ju,  K.S.    Pister,  and  R.L.    Taylor,  “An  Assessment  of  the  Cap  Model: 
Consistent  Return  Algorithms  and  Rate-Dependent  Extension,”  J.    Eng.    Mech., 
Vol.  114, No.  2, 191-218 (1988a).
REFERENCES 
Simo,  J.C.,  J.W.    Ju,  K.S.    Pister,  and  R.L.    Taylor,  “Softening  Response,  Completeness 
Condition, and Numerical Algorithms for the Cap Model,” Int.  J.  Numer.  Analy.  
Meth.  Eng., (in press) (1988b). 
Simo, J.  C., J.W.  Ju, K.S.  Pister, and R.L.  Taylor, “Softening Response, Completeness 
Condition, and Numerical Algorithms for the Cap Model,” Int.  J.  Numer.  Analy.  
Meth.  Eng.  (1990). 
Solberg,  J.M.,  and  C.M.    Noble,  “Contact  Algorithm  for  Small-Scale  Surface  Features 
with  Application  to  Finite  Element  Analysis  of  Concrete  Arch  Dams  with 
Beveled Contraction Joints”, Lawrence Livermore National Laboratory (2002).   
Spanos, P.D.  and Tsavachidis, S., “Deterministic and stochastic analyses of a nonlinear 
system  with  a  Biot  visco-elastic  element,”  Earthquake  Engineering  and  Structural 
Dynamics, vol.  30, pp.  595–612, (2001). 
Steinberg, D.J.  and M.W.  Guinan, A High-Strain-Rate Constitutive Model for Metals, 
University of California, Lawrence Livermore National Laboratory, Rept.  UCRL-
80465 (1978). 
Steinberg, D.J.  and C.M.  Lund, “A Constitutive Model for Strain Rates form 10-4 to 106 
S-1,” J.  Appl.  Phys., 65, p.  1528 (1989). 
Stillman, D.W.  and J.O.  Hallquist, INGRID: A Three-Dimensional Mesh Generator for 
Modeling  Nonlinear  Systems,  University  of  California,  Lawrence  Livermore 
National Laboratory, Rept.  UCID-20506.  (1985). 
Stojko,  S.,  privated  communication,  NNC  Limited,  Engineering  Development  Center 
(1990). 
Stahlecker Z., Mobasher B., Rajan S.D., Pereira J.M., “Development of reliable modeling 
methodologies  for  engine  fan  blade  out  containment  analysis.    Part  II:  Finite 
element analysis”, International Journal of Impact Engineering, Volume 36, Issue 
3, Pages 447-459, (2009) 
Storakers,  B.,  “On  material  representation  and  constitutive  branching  in  finite 
compressible elasticity”, J.  Mech.  Phy.  Solids, 34 No.  2, 125-145 (1986). 
Stouffer and Dame, Inelastic Deformation of Metals, Wiley, (1996). 
Stout, M.G., D.E.  Helling, T.L.  Martin, and G.R.  Canova, Int.  J.  Plasticity, Vol.  1, pp.  
163-174, (1985). 
Structural  Engineers  Association  of  California,  Tentative  Lateral  Force  Requirements, 
Seismology Committee, SEAOC, 1974, 1990, 1996.
REFERENCES 
Sussman,  T. 
  and  Bathe,  K.J.,  “A  Finite  Element  Formulation  for  Nonlinear 
Incompressible  Elastic  and  Inelastic  Analysis,”  Computers  &  Structures,  26, 
Number 1/2, 357-409 (1987). 
Tabiei, A.  and I.  Ivanov, “Computational micro-mechanical Model of Flexible Woven 
Fabric for Finite Element Impact Simulation,” IJNME, 53, (6), 1259-1276, (2002). 
Tahoe  User  Guide,  Sandia  National  Laboratory,  can  be  downloaded 
from: 
www.sandia.gov, Input version 3.4.1, (2003). 
Taylor,  L.M.    and  D.P.    Flanagan,  PRONTO3D  A  Three-Dimensional  Transient  Solid 
Dynamics Program, Sandia Report: SAND87-1912, UC-32, (1989). 
Taylor,  R.L.    Finite  element  analysis  of  linear  shell  problems,  in  Whiteman,  J.R.    (ed.), 
Proceedings of the Mathematics in Finite Elements and Applications, Academic 
Press, New York, 191-203, (1987). 
Taylor, R.L.  and Simo, J.C.  Bending and membrane elements for the analysis of thick 
and thin shells, Proc.  of NUMETA Conference, Swansea (1985). 
Tsai, S.W.  and E.M.  Wu, “A General Theory of Strength for Anisotropic Materials,” J.  
Composite Materials, 5, pp.  73-96 (1971). 
Tuler,  F.R.    and  B.M.    Butcher,  “A  Criterion  for  the  Time  Dependence  of  Dynamic 
Fracture,” The International Journal of Fracture Mechanics, Vol.  4, No.  4, (1968). 
Tvergaard,  V.    and  J.W.    Hutchinson,  “The  relation  between  crack  growth  resistance 
and fracture process parameters in elastic-plastic solids,” J.  of the Mech.  And Phy.  
of Solids, 40, pp1377-1397, (1992) 
Tvergaard, V.  and Needleman, A., “Analysis of the cup-cone fracture in a round tensile 
bar”, Acta Metallurgica, 32, 157-169 (1984).   
Vawter,  D.,  “A  Finite  Element  Model  for  Macroscopic  Deformation  of  the  Lung,” 
published in the Journal of Biomechanical Engineering, Vol.102, pp.  1-7 (1980). 
VDA Richtlinier (Surface Interfaces), Version 20, Verband der Automobilindustrie e.v., 
Frankfurt, Main, Germany, (1987). 
Vegter,  H.,  Horn,  C.H.L.J.    ten,  An,  Y.,  Atzema,  E.H.,  Pijlman,  H.H.,  Boogaard,  A.H.  
van  den,  Huetink,  H.,  “Characterisation  and  Modelling  of  the  Plastic  Material 
Behaviour and its Application in Sheet Metal Forming Simulation”, Proceedings of 
7th  International  Conference  on  Computational  Plasticity  COMPLAS  VII,  Barcelona 
(2003).
REFERENCES 
Vegter, H., and Boogaard, A.H.  van den, “A plane stress yield function for anisotropic 
sheet  material  by  interpolation  of  biaxial  stress  states”,  International  Journal  of 
Plasticity 22, 557-580 (2006). 
Walker,  J.C.,  Ratcliffe  M.B.,  Zhang  P.,  Wallace  A.W.,  Fata,  B.,  Hsu  E.,  Saloner  D.,  and 
Guccione J.M.  “MRI-based finite-element analysis of left ventricular aneurysm”, 
Am J Physiol Heart Circ Physiol 289(2): H692:700 (2005).    
Wang,  J.T.    and  O.J.    Nefske,  “A  New  CAL3D  Airbag  Inflation  Model,”  SAE  paper 
880654, 1988. 
Wang,  J.T.,  “An  Analytical  Model  for  an  Airbag  with  a  Hybrid  Inflator”,  Publication 
R&D 8332, General Motors Development Center, Warren, Mi.  (1995). 
Wang, J.T., “An Analytical Model for an Airbag with a Hybrid Inflator”, AMD-Vol.  210, 
BED-Vol.  30, ASME, pp 467-497, (1995). 
Wang,  K.,  Y.    J.    Chao,  Y.    J.,  X.    Zhu.,  and  K.W.    Miller  “Dynamic  Separation  of 
Resistance  Spot  Welded  Joints:  Part  II—Analysis  of  Test  Results  and  a  Model” 
Exp Mech Vol 50, Issue 7, pp 901-913 (2010). 
Weiss,  J.A.,  Maker,  B.N.    and  Govindjee,  S.,  “Finite  Element  Implementation  of 
Incompressible,  Transversely  Isotropic  Hyperelasticity”,  Comp.    Meth.    Appl.  
Mech.  Eng., 135, 107-128 (1996). 
Wen,  T.K.    “Method  for  Random  Vibration  of  Hysteretic  Systems”,  J.    Engrg.    Mech., 
ASCE, Vol.  102, No.  EM2, Proc.  Paper 12073, pp.249-263 (1976). 
Whirley,  R.    G.,  and  J.    O.    Hallquist,  DYNA3D,  A  Nonlinear,  Explicit,  Three-
Dimensional  Finite  Element  Code  for  Solid  and  Structural  Mechanics-Users 
Manual,  Report  No.UCRL-MA-107254 
,  Lawrence  Livermore  National 
Laboratory,  (1991). 
Whirley, R.  G., and G.A.  Henshall, “Creep Deformation Structural Analysis Using An 
Efficient Numerical Algorithm,” IJNME, Vol.  35, pp.  1427-1442, (1992). 
Wilkins, M.L., “Calculations of Elastic Plastic Flow,” Meth.  Comp.  Phys., 3, (Academic 
Press), 211-263 (1964). 
Wilkins,  M.L.,  Calculation  of  Elastic-Plastic  Flow,  University  of  California,  Lawrence 
Livermore National Laboratory, Rept.  UCRL-7322, Rev.  I (1969). 
Wilkins,  M.L.,  The  Use  of  Artificial  Viscosity  in  Multidimensional  Fluid  Dynamics 
Calculations, University of California, Lawrence Livermore National Laboratory, 
Rept.  UCRL-78348 (1976)
REFERENCES 
Wilkins, M.L., R.E.  Blum, E.  Cronshagen, and P.  Grantham, A Method for Computer 
Simulation  of  Problems  in  Solid  Mechanics  and  Gas  Dynamics  in  Three 
Dimensions  and  Time,  University  of  California,  Lawrence  Livermore  National 
Laboratory, Rept.  UCRL-51574 (1974). 
Wilkins,  M.L.,  J.E.    Reaugh,  B.    Moran,  J.K.    Scudder,  D.F.    Quinones,  M.E.    Prado, 
Fundamental Study of Crack Initiation and Propagation Annual Progress Report, 
Report  UCRL-52296,  Lawrence  Livermore  National  Laboratory,  Livermore,  CA.  
(1977). 
Wilkins, M.L, Streit, R.D, and Reaugh, J.E. Cumulative-Strain-Damage Model of Ductile 
Fracture: Simulation and Prediction of Engineering Fracture Tests, Report UCRL-
53058, Lawrence Livermore National Laboritory, Livermore, CA (1980). 
Williams  K.    V.,  Vaziri  R.,  Poursartip  A.,  “A  Physically  Based  Continuum  Damage 
Mechanics Model for Thin Laminated Composite Structures.” Int J Solids Struct, 
Vol 40(9), 2267-2300 
Wilson, E.L. Three Dimensional Static and Dynamic Analysis of Structures, Computers and 
Structures, Inc., Berkeley CA, (2000). 
Winters,  J.M.,  “Hill-based  muscle  models:    A  systems  engineering  perspective,”  In 
Multiple  Muscle  Systems:    Biomechanics  and  Movement  Organization,  JM 
Winters and SL-Y Woo eds, Springer-Verlag (1990). 
Winters  J.M.    and  Stark  L.,  “Estimated  mechanical  properties  of  synergistic  muscles 
involved  in  movements  of  a  variety  of  human  joints,”  J  Biomechanics  21:1027-
1042, (1988). 
Woodruff,  J.P.,  KOVEC  User's  Manual,  University  of  California,  Lawrence  Livermore 
National Laboratory, Report UCRL-51079, (1973). 
Worswick,  M.J.,  and  Xavier  Lalbin,  Private  communication,  Livermore,  California, 
(1999). 
Wu  Y.,  John  E.    Crawford,  Shengrui  Lan,  and  Joseph  M.,  “Validation  studies  for 
concrete  constitutive  models  with  blast  test  data”,  13th  International  LS-DYNA 
User’s Conference, Dearborn MI, (2014). 
Xia,  Q.S.,  M.C.    Boyce,  and  D.M.    Parks,  “A  constitutive  model  for  the  anisotropic 
elasticplastic deformation of paper and paperboard,” Int.  J.  Solids and Struct., 39, 
4053-4071 (2002).  
Yamasaki, H., M.  Ogura, R.  Nishimura, and K.  Nakamura, “Development of Material 
Model for Crack Propagation of Casting Aluminum”, Presented at the 2006 JSAE 
Annual Congress, Paper Number 20065077, (2006).
REFERENCES 
Yen,  C.F.,  “Ballistic  Impact  Modeling  of  Composite  Materials”,  Proceedings  of  the  7th 
International LS-DYNA Users Conference, Dearborn, MI, May 19-21, 2002, 6.15-
6.25. 
Yoshida, F.  and Uemori, T., “A Model of Large-Strain Cyclic Plasticity Describing the 
Bauschinger  Effect  and  Work  Hardening  Stagnation”,  International  Journal  of 
Plasticity 18, 661-686 (2002). 
Yoshida,  F.    and  Uemori,  T.,  “A  Model  of  Large-Strain  Cyclic  Plasticity  and  its 
Application  to  Springback  Simulation”,  International  Journal  of  Mechanical 
Sciences, Vol.  45, 1687-1702, (2003). 
Zajac  F.E.,  “Muscle  and  tendon:    Properties,  models,  scaling,  and  application  to 
biomechanics and  motor control”, CRC Critical Reviews in Biomedical Engineering 
17(4):359-411, (1989). 
Zayas, V.A., Low, S.S.  and Mahin, S.A., “A Simple Pendulum Technique for Achieving 
Seismic Isolation”, J.  Earthquake Spectra, Vol.  6, No.  2, pp.  317-334 (1990). 
Zhang, S., Approximate Stress Intensity Factors and Notch Stresses for Common Spot-
Welded Specimens, Welding Research Supplement, pp.  173s-179s, (1999). 
Zhang,  S.,  McCormick,  P.G.,  Estrin,  Y.,  “The  morphology  of  Portevin-Le  Chatelier 
bands:  Finite  element  simulation  for  Al-Mg-Si”,  Acta  Materialia  49,  1087-1094, 
(2001).
APPENDIX A 
APPENDIX A:  User Defined Materials 
Getting Started with User Defined Features 
As  a  way  of  entering  the  topic,  we  begin  by  giving  a  general  introduction  to  User 
Defined  Features  (UDF)  in  general.    This  section  is  supposed  to  be  valid  for  any  UDF 
described in the remaining appendices and serves as a practical guide to get to the point 
where technical coding may commence.  For a comprehensive overview of UDFs and its 
applications,  please  refer  to  Erhart  [2010]  which  can  be  seen  as  a  complement  to  the 
present text. 
Object 
version 
lsdyna_...tgz 
lsdyna ...zip
Unpacking to usermat
Compiler (external) 
Intel Fortran (IFC) 
Portland Groups (PGI) 
GNU (for shared libs 
and modules)
Libraries 
libdyna.a 
libmf2.a 
etc 
Includes
nhisparm.inc 
memaia.inc 
etc 
Source
dyn21.F 
dyn21b.F 
etc 
Makefile 
Download 
The  first  thing  to  do  is  to  download  an  object  version  of  LS-DYNA  for  the  computer 
architecture/platform  of  interest.    This  is  a  compressed  package  (.tgz,.tar.gz,.zip) 
provided  by  your  local  LS-DYNA  distributor  whose  unpacked  content  is  not  only  a 
single binary executable but a usermat directory possibly including 
•precompiled static object libraries (.a, .lib) 
•fortran source code files (.f, .F) 
•include files (.inc) 
•makefile 
It is important to know what version to download, i.e., a version that is compatible with 
your  computer  environment  in  terms  of  architecture,  operating  system  and  possible 
MPI  implementation  in  case  of  MPP.    This  may  not  be  obvious  to  all  users  and  for 
questions regarding this we refer to your LS-DYNA distributor.  An object version does 
not  require  a  special  license  but  goes  under  the  general  LS-DYNA  license  agreement.  
The picture above gives a conceptual overview of the usermat package, and at this point
APPENDIX A 
we need to mention that presence of libraries and include files are made obsolete with 
the  advent  of  modules  as  to  be  explained  below,  but  we  start  with  the  non-modular 
approach. 
Static or Dynamic linking 
To get something that is actually runnable it is necessary to compile the source code files 
and  link  the  resulting  object  files  either  to  a  shared  object  (.so,  .dll)  or  with  the 
precompiled libraries to a binary executable.  The former option requires a shared object 
version of the usermat package while the latter assumes a statically linked version, and 
this is thus a choice that needs to be made before retrieving the package.  Working with 
shared objects is more flexible in the sense that a binary executable can be installed once 
and  for  all  and  the  (small)  shared  object  is  dynamically  linked  at  runtime  as  a  plugin.  
Upon execution, LS-DYNA will look for the shared object file in directories specified by 
a library path that is usually set/edited in the run command script, and when found the 
shared  object  content  is  linked  to  the  execution.    On  Linux  OS’s  this  is  for  instance 
governed  by  the  environment  variable  LD_LIBRARY_PATH.    The  shared  object  is 
easily substituted or the run command script can be edited to redirect the location of the 
shared  object,  and  this  facilitates  portability  when  working  on  large  projects.    A 
statically  linked  version  requires  that  the  entire  binary  executable  is  generated  at 
compile time and this  option may be preferred if  working on small projects or during 
the development phase. 
Compiler and Compiling 
The  compilation  is  usually  performed  in  the  usermat  (working)  directory  using  a 
terminal window.  The object version does not contain a compiler but it is assumed that 
the appropriate compiler is installed on your system and accessible from your working 
directory.    To  render  compatibility  between  the  precompiled  libraries  or  binary 
executable  and  your  compiled  object  files,  the  appropriate  compiler  is  the  (by  LSTC) 
designated  compiler  with  which  the  precompiled  libraries  or  binary  are  readily 
compiled.    As  examples,  on  Linux  this  is  typically  either  the  Intel  Fortran  Compiler 
(IFC)  on  Red  Hat  or  CentOS  or  Portland  Groups  Compiler  (PGF)  on  SUSE,  and  on 
Windows  it  is  the  Intel  Fortran  Compiler  (IFC)  in  combination  with  Microsoft  Visual 
Studio  (MSVS).   For MPP  you  also  need  a wrapper  for  whatever  MPI  implementation 
you  have  installed,  but  again,  consult  your  LS-DYNA  distributor  for  detailed 
information. 
To compile, execute ‘make’ in the terminal window and in most cases this will generate 
a  shared  object  or  binary  executable  depending  on  your  type  of  LS-DYNA  object 
version, and if not it comes down to interpreting error messages.  A possible reason for 
failure  is  that  the  makefile  that  comes  with  the  usermat  package  does  not  contain 
appropriate  compiler  directives  and  requires  some  editing.    This  could  range  from 
trivial tasks like altering the path used to actually find the compiler on your system to 
more  complex  endeavors  such  as  adding  or  changing  compiler  flags.    An  even  worse 
scenario is that your operating system is not up-to-date and may require that the library 
content  on  your  computer  is  somehow  updated.    Whatever  the  reason  might  be,  any
APPENDIX A 
case is unique and the situation is preferrably resolved by your computer administrator 
in collaboration with your LS-DYNA distributor. 
Execution 
When  compiling  a  virgin  instance  of  an  object  version,  the  generated  executable 
{xyz}dyna in combination with a possible shared object lib{xyz}dyna_{t}_{Y}.{Z}.so makes 
up  an  exact  replica  of a  non-object  executable  counterpart.    It  is  only  when  the  source 
code  is  modified  that  a  customized  version  is  generated.    In  the  adopted  binary  and 
shared object naming convention above, xyz stands for smp or mpp, t is either s for single 
precision or d for double precision, Y is the base revision number for the LS-DYNA and 
Z is the corresponding release revision number. Z is always larger than Y.  The binary 
and shared object may be left in the working directory, moved to some other location on 
your  system  or  properly  installed  for  execution  on  clusters  by  a  queuing  system.  
Obviously the way execution is performed is affected accordingly, and we don’t claim 
to cover all these situations but leave this task to you and your computer administrator.  
While  the  executable  may  be  renamed,  a  shared  object  should  in  general  not  be  since 
this dynamic dependence is built into the executable.  During the development phase it 
may be convenient to leave the binary in its place to facilitate debugging, but possibly 
move the shared object to the execution directory to not having to edit the library path 
for the executable to find it.  Two Linux examples on how to run an input file are given 
in the following, one assuming an SMP static object version has been downloaded and 
the other an MPP shared object version.  Let /path_to_my_source/usermat be the complete 
path to the working directory and in.k be the name of the LS-DYNA keyword input file.  
If located in the execution directory, i.e., the directory containing in.k, the problem is run 
as 
/path_to_my_source/usermat/lsdyna i = in.k 
in the SMP case.  For the MPP shared object case, you may copy the shared object file to 
the execution directory which is a default directory for executables to look for dynamic 
object files.  Assuming the MPI software is platform-MPI, the input file could be run on 
2 cores as 
/path_to_platform-mpi/bin/mpirun –np 2  /path_to_my_source/usermat/mppdyna i = in.k 
These  two  examples  are  only  intended  to  indicate  how  to  treat  the  compiled  files  and 
changes in details thereof are to be expected. 
Coding 
All subroutines for the UDFs are collected in the files dyn21.f and dyn21b.f and are ready 
for  editing  using  your  favorite  text  editor.    Mechanical  user  materials,  user  defined 
loading,  user  defined  wear  and  friction  are  contained  in  dyn21.f,  while  user  defined 
elements and thermal user materials are in dyn21b.f, just to give a few examples.  The 
prevailing programming language is Fortran 77, but many compilers support Fortran 90
APPENDIX A 
and it may also be possible to write C code but this requires some manipulation of the 
makefile and function interfaces.  Each individual feature is connected to one or a few 
keywords  to  properly  take  advantage  of  innovative  coding.    For  user  materials,  this 
keyword  is  *MAT_USER_DEFINED_MATERIAL_MODELS  and  is  described  in  detail 
below, and for user defined loads the corresponding keyword is *USER_LOADING.  We 
refer to the individual keyword sections for details on their respective usage.   
Module Concept 
As  of  version  R9  of  LS-DYNA,  there  is  yet  another  way  of  approaching  user  defined 
features, namely through the concept of modules.  The purpose is twofold; 
1.To  facilitate  working  with  UDFs  in  that  the  content  of  the  usermat  package  is 
significantly reduced and instead replaced by *MODULE keywords 
2.To enhance  flexibility when incorporating features delivered as shared objects by 
third parties 
By  way  of  1,  the  usermat  package  only  consists  of  a  makefile  and  a  few  source  code 
files, and in principle all the user needs to do is to (i) implement the feature of interest in 
the source code files, (ii) compile to a shared object using the makefile, and (iii) use the 
keyword input file to access the generated object.  A shared object to be used in this way 
is henceforth called a module.  One of two nice side effects coming out of this approach 
is that the restriction on the choice of compiler is alleviated, the source code files can be 
compiled with any valid fortran compiler as long as the generated module is linkable as 
a plug-in to LS-DYNA.  The other is that a standard LS-DYNA executable can be used to 
access the modules, i.e., it is not required to acquire a special “module” version to use 
with this approach.  To explain how LS-DYNA in practice access modulus and specific 
routines  therein,  and  at  the  same  time  address  2  above,  the  *MODULE  keyword 
requires some attention by means of an example.
APPENDIX A 
module usermat package
LS-DYNA 
standard 
executable,  smp 
or mpp
Source
edit to 
create 
feature
Makefile
for 
compiling 
Compiler 
(external) 
non-commercial is ok 
*KEYWORD 
… 
*MODULE 
… 
Compilie to module 
my_object.so
subroutine
your_object.so
subroutine 
Module 
provided 
by 
In a standard version of LS-DYNA the keywords 
*MODULE_PATH 
*MODULE_LOAD 
*MODULE_USE 
are  available,  see  the  Section  on  *MODULE  for  further  explanations  than  what  is 
provided  here.    With  reference  to  the  picture  above,  we  assume  that  my_object.so  and 
your_object.so  are  two  independently  generated  modules,  and  both  are  located  in 
directory  /path_to_modules.  We  also  assume  that  these  two  objects  contain  the  same 
routines  names,  one  of  them  being  the  source  code  for  user  material  41  (subroutine 
umat41).  Without the present approach, it would be at least intricate to execute both of 
these two source codes in the same LS-DYNA executable and same keyword input.  A 
simple way of dealing with this here is to use the following set of keywords 
*MODULE_PATH 
/path_to_modules 
*MODULE_LOAD 
$ MDLID             TITLE 
myid                my library 
$ FILENAME 
my_object.so 
*MODULE_LOAD 
$ MDLID             TITLE 
yourid              your library 
$ FILENAME 
your_object.so 
*MODULE_USE 
$ MDLID
APPENDIX A 
myid 
$ TYPE              PARAM1              PARAM2 
UMAT                1001                41 
*MODULE_USE 
$ MDLID 
yourid 
$ TYPE              PARAM1              PARAM2 
UMAT                1002                41 
*MAT_USER_DEFINED_MATERIAL_MODELS 
$       MID        RO        MT 
          1   7.85e-9      1001 
… 
*MAT_USER_DEFINED_MATERIAL_MODELS 
$       MID        RO        MT 
          2   7.85e-9      1002 
… 
*PART 
first part 
$       PID     SECID       MID 
          1         1         1 
*PART 
second part 
$       PID     SECID       MID 
          2         2         2 
The  *MODULE_PATH  lists  the  path(s)  to  the  modules  to  be  loaded,  *MODULE_LOAD 
actually  loads  the  module  into  LS-DYNA,  and  *MODULE_USE  tells  LS-DYNA  how  to 
access routines in the module.  In this particular example, the rules (TYPE = UMAT) are 
that a user material *MAT_USER_... with MT set to 1001 (because PARAM1 = 1001) 
will  execute  subroutine  umat41  (because  PARAM2 = 41)  in  the  module  with  id 
myid  (because  MDLID = myid)  and  in  the  same  manner  user  material  with  MT  set  to 
1002 will also execute subroutine umat41 but now in the module with id yourid.  
Hence we have made part 1 and part 2, in the same keyword input file, execute the same 
subroutine  (by  name)  but  in  different  modules.    Obviously  this  generalizes  to  any 
number  of  modules  by  analogy,  see  *MODULE_USE  for  many  more  rules  and  yet 
another example. 
General overview 
We  now  turn  to  the  specific  documentation  of  user  defined  materials.    Up  to  ten  user 
subroutines  can  currently  be  implemented  simultaneously  to  update  the  stresses  in 
solids,  shells,  beams,  discrete  beams  and  truss  beams.    This  text  serves  as  an 
introductory  guide  to  implement  such  a  model.    Note  that  names  of  variables  and 
subroutines below may differ from the actual ones depending on platform and current 
version of LS-DYNA. 
When the keyword *MAT_USER_DEFINED_MATERIAL_MODELS is defined for a part in 
the keyword deck, LS-DYNA calls the subroutine usrmat with appropriate input data
APPENDIX A 
for  the  constitutive  update.    This  routine  in  turn  calls  urmathn  for  2D  and  3D  solid 
elements,  urmats  for  2D  plane  stress  and  3D  shell  elements,  urmatb  for  beam 
elements, urmatd for discrete beam elements and urmatt for truss beam elements.  In 
these  routines,  which  may  be  modified  by  the  user  if  necessary,  the  following  data 
structures  are  initialized  for the  purpose of being  supplied  to  a  specific scalar  material 
subroutine. 
sig(6) –  stresses in previous time step 
eps(6) –  strain increments 
epsp –  effective plastic strain in previous time step 
hsv(*) –  history  variables  in  previous  time  step  excluding  plastic 
strain 
dt1 –  current time step size 
temper -  current temperature 
failel –  flag indicating failure of element 
If  the  vectorization  flag  is  active  (IVECT = 1)  on  the  material  card,  variables  are  in 
general stored in vector blocks of length nlq, with vector indexes ranging from lft to 
llt  ,  which  allows  for  a  more  efficient  execution  of  the  material  routine.    As  an 
example, the data structures mentioned above are for the vectorized case exchanged for  
sigX(nlq) –  stresses in previous time step 
dX(nlq) –  strain increments 
epsps(nlq) –  effective plastic strains in previous time step 
hsvs(nlq,*) –  history variables in previous time step 
dt1siz(nlq) -  current time step sizes 
temps(nlq) –  current temperatures 
failels(nlq) –  flags indicating failure of elements 
where X ranges from 1 to 6 for the different components.  Each entry in a vector block is 
associated with an element in the finite element mesh for a fix integration point.  
The  number  of  entries  in  the  history  variables  array  (indicated  by  *  in  the  above) 
matches the number of history variables requested on the material card (NHV).  Hence 
the number NHV should equal to the number of history variables excluding the effective 
plastic  strain  since  this  variable  is  given  a  special  treatment.    All  history  variables, 
including  the  effective  plastic  strain,  are  initially  zero.    Furthermore,  all  user-defined 
material  models  require  a  bulk  modulus  and  shear  modulus  for  transmitting 
boundaries, contact interfaces, rigid body constraints, and time step calculations.  This 
generally means that the length of material constants array LMC must be increased by 2 
for the storage of these parameters.  In addition to the variables mentioned above, the 
following  data  can  be  supplied  to  the  user  material  routines,  regardless  of  whether 
vectorization is used or not. 
cm(*) –  material constants array 
capa –  transverse shear correction factor for shell elements 
tt –  current time
APPENDIX A 
crv(lq1,2,*) –  array representation of curves defined in the keyword deck 
A specific material routine, umatXX in the scalar case or umatXXv in the vector case, is 
now  called  with  any  necessary  parameters  of  the  ones  above,  and  possibly  others  as 
well.  The letters XX stands for a number between 41 and 50 and matches the number 
MT on the material card.  This subroutine is written by the user, and should update the 
stresses  and  history  variables  to  the  current  time.    For  shells  and  beams  it  is  also 
necessary to determine the strain increments in the directions of constrained zero stress.  
To  be  able  to  write  different  stress  updates  for  different  elements,  the  following 
character string is passed to the user-defined subroutine 
etype –  character string that equals solid, shell, beam, dbeam or 
tbeam 
A  sample  user  subroutine  of  a  hypo-elastic  material  in  the  scalar  case  is  provided 
below.  This sample and the others below are from the dyn21.F file that is distributed 
with version R6.1. 
Sample user subroutine 41 
      subroutine umat41 (cm,eps,sig,epsp,hsv,dt1,capa,etype,tt, 
     1 temper,failel,crv,nnpcrv,cma,qmat,elsiz,idele,reject) 
c 
c****************************************************************** 
c|  Livermore Software Technology Corporation  (LSTC)             | 
c|  ------------------------------------------------------------  | 
c|  Copyright 1987-2008 Livermore Software Tech.  Corp             | 
c|  All rights reserved                                           | 
c****************************************************************** 
c 
c     isotropic elastic material (sample user subroutine) 
c 
c     Variables 
c 
c     cm(1)=first material constant, here young's modulus 
c     cm(2)=second material constant, here poisson's ratio 
c        . 
c        . 
c        . 
c     cm(n)=nth material constant 
c 
c     eps(1)=local x  strain increment 
c     eps(2)=local y  strain increment 
c     eps(3)=local z  strain increment 
c     eps(4)=local xy strain increment 
c     eps(5)=local yz strain increment 
c     eps(6)=local zx strain increment 
c 
c     sig(1)=local x  stress 
c     sig(2)=local y  stress 
c     sig(3)=local z  stress 
c     sig(4)=local xy stress 
c     sig(5)=local yz stress 
c     sig(6)=local zx stress 
c 
c     hsv(1)=1st history variable
APPENDIX A 
c     hsv(2)=2nd history variable 
c        . 
c        . 
c        . 
c        . 
c     hsv(n)=nth history variable 
c 
c     dt1=current time step size 
c     capa=reduction factor for transverse shear 
c     etype: 
c        eq."solid" for solid elements 
c        eq."sld2d" for shell forms 13, 14, and 15 (2D solids) 
c        eq."shl_t" for shell forms 25, 26, and 27 (shells with thickness 
c         stretch) 
c        eq."shell" for all other shell elements plus thick shell forms 1 
c         and 2 
c        eq."tshel" for thick shell forms 3 and 5 
c        eq."hbeam" for beam element forms 1 and 11 
c        eq."tbeam" for beam element form 3 (truss) 
c        eq."dbeam" for beam element form 6 (discrete) 
c        eq."beam " for all other beam elements 
c 
c     tt=current problem time. 
c 
c     temper=current temperature 
c 
c     failel=flag for failure, set to .true.  to fail an integration point, 
c            if .true.  on input the integration point has failed earlier 
c 
c     crv=array representation of curves in keyword deck 
c 
c     nnpcrv=# of discretization points per crv() 
c 
c     cma=additional memory for material data defined by LMCA at 
c       6th field of 2nd crad of *DATA_USER_DEFINED 
c 
c     elsiz=characteristic element size 
c      
c     idele=element id 
c 
c     reject (implicit only) = set to .true.  if this implicit iterate is 
c                              to be rejected for some reason 
c 
c     All transformations into the element local system are 
c     performed prior to entering this subroutine.  Transformations 
c     back to the global system are performed after exiting this 
c     routine. 
c 
c     All history variables are initialized to zero in the input 
c     phase.  Initialization of history variables to nonzero values 
c     may be done during the first call to this subroutine for each 
c     element. 
c 
c     Energy calculations for the dyna3d energy balance are done 
c     outside this subroutine. 
c 
      include 'nlqparm' 
      include 'bk06.inc' 
      include 'iounits.inc' 
      dimension cm(*),eps(*),sig(*),hsv(*),crv(lq1,2,*),cma(*) 
      integer nnpcrv(*) 
      logical failel,reject 
      character*5 etype 
c 
      if (ncycle.eq.1) then 
        if (cm(16).ne.1234567) then
APPENDIX A 
          call usermsg('mat41') 
        endif 
      endif 
c 
c     compute shear modulus, g 
c 
      g2 =abs(cm(1))/(1.+cm(2)) 
      g  =.5*g2 
c 
      if (etype.eq.'solid'.or.etype.eq.'shl_t'.or. 
     1     etype.eq.'sld2d'.or.etype.eq.'tshel') then 
        if (cm(16).eq.1234567) then 
          call mitfail3d(cm,eps,sig,epsp,hsv,dt1,capa,failel,tt,crv) 
        else 
          if (.not.failel) then 
          davg=(-eps(1)-eps(2)-eps(3))/3. 
          p=-davg*abs(cm(1))/(1.-2.*cm(2)) 
          sig(1)=sig(1)+p+g2*(eps(1)+davg) 
          sig(2)=sig(2)+p+g2*(eps(2)+davg) 
          sig(3)=sig(3)+p+g2*(eps(3)+davg) 
          sig(4)=sig(4)+g*eps(4) 
          sig(5)=sig(5)+g*eps(5) 
          sig(6)=sig(6)+g*eps(6) 
          if (cm(1).lt.0.) then 
            if (sig(1).gt.cm(5)) failel=.true. 
          endif 
          endif 
        end if 
c 
      else if (etype.eq.'shell') then 
        if (cm(16).eq.1234567) then 
          call mitfailure(cm,eps,sig,epsp,hsv,dt1,capa,failel,tt,crv) 
        else 
          if (.not.failel) then 
          gc    =capa*g 
          q1    =abs(cm(1))*cm(2)/((1.0+cm(2))*(1.0-2.0*cm(2))) 
          q3    =1./(q1+g2) 
          eps(3)=-q1*(eps(1)+eps(2))*q3 
          davg  =(-eps(1)-eps(2)-eps(3))/3. 
          p     =-davg*abs(cm(1))/(1.-2.*cm(2)) 
          sig(1)=sig(1)+p+g2*(eps(1)+davg) 
          sig(2)=sig(2)+p+g2*(eps(2)+davg) 
          sig(3)=0.0 
          sig(4)=sig(4)+g *eps(4) 
          sig(5)=sig(5)+gc*eps(5) 
          sig(6)=sig(6)+gc*eps(6) 
          if (cm(1).lt.0.) then 
            if (sig(1).gt.cm(5)) failel=.true. 
          endif 
          endif 
        end if 
      elseif (etype.eq.'beam ' ) then 
          q1    =cm(1)*cm(2)/((1.0+cm(2))*(1.0-2.0*cm(2))) 
          q3    =q1+2.0*g 
          gc    =capa*g 
          deti  =1./(q3*q3-q1*q1) 
          c22i  = q3*deti 
          c23i  =-q1*deti 
          fac   =(c22i+c23i)*q1 
          eps(2)=-eps(1)*fac-sig(2)*c22i-sig(3)*c23i 
          eps(3)=-eps(1)*fac-sig(2)*c23i-sig(3)*c22i 
          davg  =(-eps(1)-eps(2)-eps(3))/3. 
          p     =-davg*cm(1)/(1.-2.*cm(2)) 
          sig(1)=sig(1)+p+g2*(eps(1)+davg) 
          sig(2)=0.0 
          sig(3)=0.0
APPENDIX A 
          sig(4)=sig(4)+gc*eps(4) 
          sig(5)=0.0 
          sig(6)=sig(6)+gc*eps(6) 
c 
      elseif (etype.eq.'tbeam') then 
        q1    =cm(1)*cm(2)/((1.0+cm(2))*(1.0-2.0*cm(2))) 
        q3    =q1+2.0*g 
        deti  =1./(q3*q3-q1*q1) 
        c22i  = q3*deti 
        c23i  =-q1*deti 
        fac   =(c22i+c23i)*q1 
        eps(2)=-eps(1)*fac 
        eps(3)=-eps(1)*fac 
        davg  =(-eps(1)-eps(2)-eps(3))/3. 
        p     =-davg*cm(1)/(1.-2.*cm(2)) 
        sig(1)=sig(1)+p+g2*(eps(1)+davg) 
        sig(2)=0.0 
        sig(3)=0.0 
c 
      else 
c       write(iotty,10) etype 
c       write(iohsp,10) etype 
c       write(iomsg,10) etype 
c       call adios(TC_ERROR) 
        cerdat(1)=etype 
        call lsmsg(3,MSG_SOL+1150,ioall,ierdat,rerdat,cerdat,0) 
      endif 
c 
c10   format(/ 
c    1 ' *** Error element type ',a,' can not be', 
c    2 '           run with the current material model.') 
      return 
      end 
Based on the subroutine umat41 shown above, the following material input… 
*MAT_USER_DEFINED_MATERIAL_MODELS 
$#     mid        ro        mt       lmc       nhv    iortho     ibulk        ig 
         1 7.8300E-6        41         4         0         0         3         4 
$#   ivect     ifail    itherm    ihyper      ieos 
         0         0         0         0         0 
$        E        PR      BULK         G 
$#      p1        p2        p3        p4        p5        p6        p7        p8 
  2.000000  0.300000  1.667000  0.769200     0.000     0.000     0.000     0.000 
… is functionally equivalent to … 
*MAT_ELASTIC 
$#     mid        ro         e        pr        da        db  not used 
         1 7.8300E-6  2.000000  0.300000     0.000     0.000         0
APPENDIX A 
Load curves and tables 
ADDITIONAL FEATURES 
If the material of interest should require load curves, for instance a curve defining yield 
stress as a function of effective plastic strain, curve and table lookup are easily obtained 
by predefined routines.   
The routines to be called are 
subroutine crvval(crv,nnpcrv,eid,xval,yval,slope) 
and 
subroutine crvval_v(crv,nnpcrv,eid,xval,yval,slope,lft,llt) 
where the former routine is used in the scalar context and the latter for vectorized umat.  
The arguments are the following 
crv -  the load curve array (available in material routine, just pass 
on) 
nnpcrv -  curve  data  pointer  (available  in  material  routine,  just  pass 
on) 
eid -  external load curve ID, i.e., the load curve ID taken from the 
keyword deck 
.GT.0:  Use approximate representation of curve 
.LT.0:  Use exact representation of curve (with id –eid) 
xval -  abscissa value 
yval -  ordinate value (output from routine) 
slope -  slope of curve (output from routine) 
lft -  first index of vector 
llt -  final index of vector 
where  xval,  yval  and  slope  are  scalars  in  the  scalar  routine  and  vectors  of  length 
nlq  in  the  vectorized  routine.    Note  that  eid  should  be  passed  as  float.    Using  a 
positive  number  for  eid  will  use  the  approximative  representation  of  the  curve, 
whereas  if  eid  is  a  negative  number  the  extraction  will  be  made  on  the  curve  as  it  is 
defined in the keyword input deck. 
For tables, two subroutines are available for extracting values.  A scalar version is 
       subroutine tabval(crv,nnpcrv,eid,dxval,yval,dslope,xval,slope) 
and a vector version is 
       subroutine  
      1 tabval_v(crv,nnpcrv,eid,dxval,yval,dslope,lft,llt,xval,slope) 
where 
crv -  curve array (available in material routine, just pass on) 
nnpcrv -  curve pointer  (available in material routine, just pass on)
APPENDIX A 
eid -  external  table  id  (data  type  real),  i.e.,  table  id  taken  from 
keyword deck  
  GT.0: Use approximative representation of curve 
LT.0:  Use exact representation of curve (with id –eid) 
dxval -  abscissa value (x2-axis) 
yval -  ordinate value (y-axis, output from routine) 
dslope -  slope of curve (dy/dx2, output from routine) 
xval -  abscissa value (x1-axis) 
slope -  slope of curve (dy/dx1, output from routine) 
lft -  vector index 
llt -  vector index 
In  the  scalar  routine,  dxval,  yval,  dslope,  xval  and  slope  are  all  scalars  whereas  in  the 
vector  routine  they  are  vectors  of  length  nlq.    Also  here,  using  a  positive  number  for 
eid will use the approximative representation of the table, whereas if eid is a negative 
number  the  extraction  will  be  made  on  the  table  as  it  is  defined  in  the  keyword  input 
deck. 
Local coordinate system 
If  the  material  model  has  directional  properties,  such  as  composites  and  anisotropic 
plasticity  models,  the  local  coordinate  system  option  can  be  invoked.    This  is  done  by 
putting IORTHO equal to 1 on the material card.  This also requires two additional cards 
with values for how the coordinate system is formed and updated.  When this option is 
used,  all  data  passed  to  the  constitutive  routine  umatXX  or  umatXXv  is  in  the  local 
system  and  the  transformation  back  to  the  global  system  is  done  outside  this  user-
defined  routine.    There  is  one  exception  however,  see  the  section  on  the  deformation 
gradient. 
Temperature 
For a material with thermal properties, temperatures are made available by putting the 
flag ITHERMAL equal to 1 on the material card.  The temperatures in the elements are 
then  available  in  the temper  variable  for  a  scalar  and temps  array  for  the  vectorized 
implementation.    For  a  coupled  thermal  structural  analysis,  the  thermal  problem  is 
solved  first  and  temperatures  at  the  current  time  are  available  in  the  user-defined 
subroutine.    Calculation  of  dissipated  heat  in  the  presence  of  plastic  deformation  is 
taken  care  of  by  LS-DYNA  and  needs  not  be  considered  by  the  user.    If  the  time 
derivative  of  the  temperature  is  needed  for  the  stress  update,  a  history  variable  that 
contains  the  temperature  in  the  previous  time  step  should  be  requested.    The  time 
derivative can then be obtained by a backward finite difference estimate.
APPENDIX A 
Failure 
It  is  possible  to  include  failure  in  the  material  model,  resulting  in  the  deletion  of 
elements that fulfill a certain failure criterion.  To accomplish this, the flag IFAIL must 
be set to 1 or a negative number on the material card.  For a scalar implementation, the 
variable  failel  is  set  to  .true.  when  a  failure  criterion  is  met.    For  a  vectorized 
implementation, the corresponding entry in the failels array is set to .true. 
Deformation gradient 
For  some  materials,  the  stresses  are  not  obtained  from  incremental  strains,  but  are 
expressed  in  terms  of  the  deformation  gradient  𝐅.  This  is  the  case  for  hyper-elastic(-
plastic) materials.  To make the deformation gradient available for bricks and shells in 
the user-defined material subroutines, the variable IHYPER on the material card should 
be  set  to  1.    The  deformation  gradient  components  𝐹11,  𝐹21,  𝐹31,  𝐹12,  𝐹22,  𝐹32,  𝐹13, 𝐹23 
and  𝐹33can  then  be  found  in  the  history  variables  array  in  positions  NHV+1  to  NHV+9, 
i.e., the positions coming right after the requested number of history variables. 
For shell elements, the components of the deformation gradient are with respect to the 
co-rotational  system  for  the  element  currently  used.    In  this  case  the  third  row  of  the 
deformation  gradient,  i.e.,  the  components  𝐹31,  𝐹32  and  𝐹33,  will  not  be  properly 
updated  when  entering  the  user-defined  material  routine.    These  components  depend 
on the thickness strain increment which in turn must be determined so that the normal 
stress  in  the  shell  vanishes.    For  a  given  thickness  strain  increment  d3,  these  three 
components, f31, f32 and f33, can be determined by calling the subroutine 
       subroutine compute_f3s(f31,f32,f33,d3) 
for a scalar implementation and 
       subroutine compute_f3(f31,f32,f33,d3,lft,llt) 
for a vector implementation.  The first four arguments are arrays of length nlq for the 
vector routine and scalars for the scalar routine. 
For  hyper-elastic  materials  there  are  push  forward  operations  that  can  be  called  from 
within the user defined subroutines. These are 
       subroutine push_forward_2(sig1,sig2,sig3,sig4,sig5,sig6, 
f11,f21,f31,f12,f22,f32,f13,f23,f33,lft,llt) 
which  performs a push forward operation on the stress tensor, and the corresponding 
scalar routine 
       subroutine push_forward_2s(sig1,sig2,sig3,sig4,sig5,sig6, 
f11,f21,f31,f12,f22,f32,f13,f23,f33) 
In the latter subroutine all arguments are scalars whereas the corresponding entries in 
the vectorized routine are vectors of length nlq.  The sig1 to sig6 are components of 
the stress tensor and f11 to f33 are components of the deformation gradient.
APPENDIX A 
If  the  local  coordinate  system  option  is  invoked  (IORTHO = 1),  then  the  deformation 
gradient is transformed to this local system prior to entering the user-defined material 
routine according to 
𝑠 𝐹𝑘𝑗 
𝑠   refers  to  a  transformation  between  the  current  global  and  material  frames.  
where  𝑄𝑖𝑗
For IORTHO equal to 1 one can choose to put IHYPER equal to –1 which results in that 
the deformation gradient is transformed according to 
𝐹̅𝑖𝑗 = 𝑄𝑘𝑖
𝑟  
𝐹̅𝑖𝑗 = 𝐹𝑖𝑘𝑄𝑘𝑗
𝑟  is the transformation between the reference global and material and frames.  
where 𝑄𝑖𝑗
For this latter option the spatial frame remains the global one so the stresses should be 
expressed  in  this  frame  of  reference  upon  exiting  the  user  defined  routines.    The 
suitable choice of IHYPER depends on the formulation of the material model. 
For shells, there is also the special option of setting IHYPER = 3 which will make the 
deformation  gradient  computed  from  the  nodal  coordinates  and  in  the  global 
coordinate  system.    With  this  option  the  user  must  compute  the  stress  in  the  local 
system  of  interest,  whence  a  transformation  matrix  between  the  global  and  this  local 
system  is  passed  to  the  user  material  routines  (qmat).    The  columns  in  this  matrix 
correspond to local basis vectors expressed in global coordinates, and this is the system 
that stress needs to be computed in.  The user must be aware that since the deformation 
gradient  is  calculated  directly  from  the  element  deformation  it  may  not  be  consistent 
with  the  theory  of  the  element  that  is  used  for  the  material.    To  account  for  thickness 
changes due to membrane straining, there are routines 
subroutine usrshl_updatfs(f,t,s,e) 
real f(3,3),t(4),s(4),e 
that recompute the deformation gradient based on the thickness strain increment e, and 
the  nodal  thicknesses  t.    The  current  nodal  thicknesses  are  stored  in  the  history 
variables  array  immediately  following  the  storage  of  the  deformation  gradient.    This 
routine  must  be  called  with  these  four  values  as  t.    This  subroutine  is  expected  to 
produce  a  deformation  f  and  the  new  thicknesses  s.    This  routine  is  used  to  find  the 
strain increment e giving zero thickness stress.  Once zero thickness stress is obtained, 
the  user  needs  to  store  the  new  thicknesses  s  in  the  history  variables  array,  which  is 
achieved  by  copying  the  new  thicknesses  s  to  the  location  for  the  nodal  thicknesses.  
There  is  also  a  vectorized  version  of  this  routine  called  usrshl_updatfv.    Sample 
code is provided in the object library. 
In  the  following,  a  Neo-Hookean  material  is  used  as  an  example  of  the  usage  of  the 
deformation  gradient  in  user-defined  materials.    With  𝜆  and  𝜇  being  the  Lame 
parameters in the linearized theory, the strain energy density for this material is given 
by
APPENDIX A 
𝜓 =
𝜆(ln(det𝐅))2 − 𝜇ln(det𝐅) +
𝜇(tr(𝐅𝑇𝐅) − 3) 
meaning that the Cauchy stress can be expressed as 
σ =
det𝐅
(𝜆ln(det𝐅)𝐈 + 𝜇(𝐅𝐅𝑇 − 𝐈)). 
Sample user subroutine 45 
      subroutine umat45 (cm,eps,sig,epsp,hsv,dt1,capa, 
     .  etype,time,temp,failel,crv,nnpcrv,cma,qmat,elsiz,idele,reject) 
c 
c****************************************************************** 
c|  Livermore Software Technology Corporation  (LSTC)             | 
c|  ------------------------------------------------------------  | 
c|  Copyright 1987-2008 Livermore Software Tech.  Corp             | 
c|  All rights reserved                                           | 
c****************************************************************** 
c 
c     Neo-Hookean material (sample user subroutine) 
c 
c     Variables 
c 
c     cm(1)=first material constant, here young's modulus 
c     cm(2)=second material constant, here poisson's ratio 
c        . 
c        . 
c        . 
c     cm(n)=nth material constant 
c 
c     eps(1)=local x  strain increment 
c     eps(2)=local y  strain increment 
c     eps(3)=local z  strain increment 
c     eps(4)=local xy strain increment 
c     eps(5)=local yz strain increment 
c     eps(6)=local zx strain increment 
c 
c     sig(1)=local x  stress 
c     sig(2)=local y  stress 
c     sig(3)=local z  stress 
c     sig(4)=local xy stress 
c     sig(5)=local yz stress 
c     sig(6)=local zx stress 
c 
c     hsv(1)=1st history variable 
c     hsv(2)=2nd history variable 
c        . 
c        . 
c        . 
c        . 
c     hsv(n)=nth history variable 
c 
c     dt1=current time step size 
c     capa=reduction factor for transverse shear 
c     etype: 
c       eq."solid" for solid elements 
c       eq."sld2d" for shell forms 13, 14, and 15 (2D solids) 
c       eq."shl_t" for shell forms 25, 26, and 27 (shells with thickness 
c        stretch) 
c       eq."shell" for all other shell elements plus thick shell forms 1 
c        and 2
APPENDIX A 
c       eq."tshel" for thick shell forms 3 and 5 
c       eq."hbeam" for beam element forms 1 and 11 
c       eq."tbeam" for beam element form 3 (truss) 
c       eq."dbeam" for beam element form 6 (discrete) 
c       eq."beam " for all other beam elements 
c 
c     time=current problem time. 
c 
c     temp=current temperature 
c 
c     failel=flag for failure, set to .true.  to fail an integration point, 
c            if .true.  on input the integration point has failed earlier 
c 
c     crv=array representation of curves in keyword deck 
c 
c     nnpcrv=# of discretization points per crv() 
c 
c     cma=additional memory for material data defined by LMCA at 
c       6th field of 2nd crad of *DATA_USER_DEFINED 
c 
c     elsiz=characteristic element size 
c      
c     idele=element id 
c 
c     reject (implicit only) = set to .true.  if this implicit iterate is 
c                              to be rejected for some reason 
c 
c     All transformations into the element local system are 
c     performed prior to entering this subroutine.  Transformations 
c     back to the global system are performed after exiting this 
c     routine. 
c 
c     All history variables are initialized to zero in the input 
c     phase.   Initialization of history variables to nonzero values 
c     may be done during the first call to this subroutine for each 
c     element. 
c 
c     Energy calculations for the dyna3d energy balance are done 
c     outside this subroutine. 
c 
      include 'nlqparm' 
      include 'iounits.inc' 
      include 'bk06.inc' 
      character*5 etype 
      dimension cm(*),eps(*),sig(*),hsv(*),crv(lq1,2,*),cma(*) 
      logical failel 
c 
      if (ncycle.eq.1) then 
        call usermsg('mat45') 
      endif 
c 
c     compute lame parameters 
c 
      xlambda=cm(1)*cm(2)/((1.+cm(2))*(1.-2.*cm(2))) 
      xmu=.5*cm(1)/(1.+cm(2)) 
c 
      if (etype.eq.'solid'.or.etype.eq.'shl_t'.or. 
     1     etype.eq.'sld2d'.or.etype.eq.'tshel') then 
c 
c       deformation gradient stored in hsv(1),...,hsv(9) 
c 
c       compute jacobian 
c 
        detf=hsv(1)*(hsv(5)*hsv(9)-hsv(6)*hsv(8)) 
     1      -hsv(2)*(hsv(4)*hsv(9)-hsv(6)*hsv(7)) 
     2      +hsv(3)*(hsv(4)*hsv(8)-hsv(5)*hsv(7))
APPENDIX A 
c 
c       compute left cauchy-green tensor 
c 
        b1=hsv(1)*hsv(1)+hsv(4)*hsv(4)+hsv(7)*hsv(7) 
        b2=hsv(2)*hsv(2)+hsv(5)*hsv(5)+hsv(8)*hsv(8) 
        b3=hsv(3)*hsv(3)+hsv(6)*hsv(6)+hsv(9)*hsv(9) 
        b4=hsv(1)*hsv(2)+hsv(4)*hsv(5)+hsv(7)*hsv(8) 
        b5=hsv(2)*hsv(3)+hsv(5)*hsv(6)+hsv(8)*hsv(9) 
        b6=hsv(1)*hsv(3)+hsv(4)*hsv(6)+hsv(7)*hsv(9) 
c 
c       compute cauchy stress 
c 
        detfinv=1./detf 
        dmu=xmu-xlambda*log(detf) 
        sig(1)=detfinv*(xmu*b1-dmu) 
        sig(2)=detfinv*(xmu*b2-dmu) 
        sig(3)=detfinv*(xmu*b3-dmu) 
        sig(4)=detfinv*xmu*b4 
        sig(5)=detfinv*xmu*b5 
        sig(6)=detfinv*xmu*b6 
c 
      else if (etype.eq.'shell') then 
c 
c       deformation gradient stored in hsv(1),...,hsv(9) 
c 
c       compute part of left cauchy-green tensor 
c       independent of thickness strain increment 
c 
        b1=hsv(1)*hsv(1)+hsv(4)*hsv(4)+hsv(7)*hsv(7) 
        b2=hsv(2)*hsv(2)+hsv(5)*hsv(5)+hsv(8)*hsv(8) 
        b4=hsv(1)*hsv(2)+hsv(4)*hsv(5)+hsv(7)*hsv(8) 
c 
c       secant iterations for zero normal stress 
c 
        do iter=1,5 
c 
c         first thickness strain increment initial guess 
c         assuming Poisson's ratio different from zero 
c 
          if (iter.eq.1) then 
            eps(3)=-xlambda*(eps(1)+eps(2))/(xlambda+2.*xmu) 
c 
c         second thickness strain increment initial guess 
c 
          else if (iter.eq.2) then 
            sigold=sig(3) 
            epsold=eps(3) 
            eps(3)=0. 
c 
c         secant update of thickness strain increment 
c 
          else if (abs(sig(3)-sigold).gt.0.0) then 
            deps=-(eps(3)-epsold)/(sig(3)-sigold)*sig(3) 
            sigold=sig(3) 
            epsold=eps(3) 
            eps(3)=eps(3)+deps 
          endif 
c 
c         compute last row of deformation gradient 
c 
          call compute_f3s(hsv(3),hsv(6),hsv(9),eps(3)) 
c 
c         compute jacobian 
c 
          detf=hsv(1)*(hsv(5)*hsv(9)-hsv(6)*hsv(8)) 
     1        -hsv(2)*(hsv(4)*hsv(9)-hsv(6)*hsv(7))
APPENDIX A 
     2        +hsv(3)*(hsv(4)*hsv(8)-hsv(5)*hsv(7)) 
c 
c         compute normal component of left cauchy-green tensor 
c 
          b3=hsv(3)*hsv(3)+hsv(6)*hsv(6)+hsv(9)*hsv(9) 
c 
c         compute normal stress 
c 
          detfinv=1./detf 
          dmu=xmu-xlambda*log(detf) 
          sig(1)=detfinv*(xmu*b1-dmu) 
          sig(2)=detfinv*(xmu*b2-dmu) 
          sig(3)=detfinv*(xmu*b3-dmu) 
          sig(4)=detfinv*xmu*b4 
c 
c         exit if normal stress is sufficiently small 
c 
          if (abs(sig(3)).le.1.e-5* 
     1     (abs(sig(1))+abs(sig(2))+abs(sig(4)))) goto 10 
         enddo 
c 
c       compute remaining components of left cauchy-green tensor 
c 
 10     b5=hsv(2)*hsv(3)+hsv(5)*hsv(6)+hsv(8)*hsv(9) 
        b6=hsv(1)*hsv(3)+hsv(4)*hsv(6)+hsv(7)*hsv(9) 
c 
c       compute remaining stress components 
c 
        sig(5)=detfinv*xmu*b5 
        sig(6)=detfinv*xmu*b6 
c 
c     material model only available for solids and shells 
c 
      else 
        cerdat(1)=etype 
        call lsmsg(3,MSG_SOL+1151,ioall,ierdat,rerdat,cerdat,0) 
      endif 
      return 
      end 
Implicit analysis 
For brick, and shell, thick shell and Hughes-Liu beam elements, a user-defined material 
model can also be run with implicit analysis.  When an implicit analysis is requested in 
the input keyword deck, LS-DYNA calls the subroutine urtanh for bricks, urtans for 
shells  and  urtanb  for  beams  with  appropriate  input  data  for  the  calculation  of  the 
material  tangent  modulus.    For  a  scalar  implementation,  this  routine  in  turn  calls 
utanXX with all necessary input parameters including 
es(6,6) –  material tangent modulus 
Again,  XX  is  the  number  that  matches  MT  on  the  material  card.    For  a  vectorized 
implementation, the routine utanXXv is called, this time with the corresponding vector 
block 
dsave(nlq,6,6) –  material tangent modulus 
This  subroutine  builds  the  tangent  modulus  to  be  used  for  assembling  the  tangent 
stiffness  matrix  and  must  be  provided  by  the  user.    This  matrix  is  equal  to  the  zero
APPENDIX A 
matrix  when  entering  the  user-defined  routine,  it  must  be  symmetric  and  if  the  local 
coordinate system option is invoked for bricks, then it should be expressed in this local 
system.  For shell elements, it should be expressed in the co-rotational system defined 
for  the  current  shell  element.    All  transformations  back  to  the global  system  are  made 
after exiting the user-defined routine.  
A  feature  that  can  be  made  useful  for  improving  convergence  characteristics  is  the 
parameter reject, which can be set to .true.  in the user material routine.  The purpose of 
this  parameter  is  to  indicate  something  that  renders  the  iteration  unacceptable.    An 
example  of  this  something  may  be  too  much  increase  in  plastic  strain  in  one  step, 
another  is  a  criterion  on  the  total  strain  increment.    What  LS-DYNA  will  do  in  this 
situation  is  to  print  a  warning  message  ‘Material  model  rejected  current  iterate’  and 
retry the step with a smaller time step.  If chosen carefully (by way of experimenting), 
this  may  result  in  a  good  trade-off  between  the  number  of  implicit  iterations  per  step 
and the step size for overall speed.  
If  the  material  is  hyper-elastic,  there  are  push  forward  operations  of  tangent  modulus 
tensor available in 
       subroutine push_forward_4(dsave,  
f11,f21,f31,f12,f22,f32,f13,f23,f33,lft,llt) 
which  performs  a  push  forward  operation  on  the  tangent  modulus  tensor,  and  the 
corresponding scalar routine 
       subroutine push_forward_4s(es, 
f11,f21,f31,f12,f22,f32,f13,f23,f33) 
In the latter subroutine all arguments are scalars whereas the corresponding entries in 
the vectorized routine are vectors of length nlq.  The f11 to f33 are components of the 
deformation gradient. 
The following sample user subroutine illustrates how to implement the tangent stiffness 
modulus for the Neo-Hookean material above.  The material tangent modulus is for this 
material given by 
𝐂 =
det𝐅
(𝜆𝐈 ⊗ 𝐈 + 2(𝜇 − 𝜆ln(det𝐅))𝐈). 
Sample user subroutine 42, tangent modulus 
      subroutine utan42(cm,eps,sig,epsp,hsv,dt1,capa, 
     .     etype,tt,temper,es,crv) 
c****************************************************************** 
c|  livermore software technology corporation  (lstc)             | 
c|  ------------------------------------------------------------  | 
c|  copyright 1987-1999                                           | 
c|  all rights reserved                                           | 
c****************************************************************** 
c 
c     Neo-Hookean material tangent modulus (sample user subroutine)
APPENDIX A 
cm(n)=nth material constant 
epsp=effective plastic strain 
c     Variables 
c      
c     cm(1)=first material constant, here young's modulus  
c     cm(2)=second material constant, here poisson's ratio 
   .      
c 
c 
   . 
c        . 
c 
c 
c     eps(1)=local x  strain increment 
c     eps(2)=local y  strain increment 
c     eps(3)=local z  strain increment 
c     eps(4)=local xy strain increment 
c     eps(5)=local yz strain increment 
c     eps(6)=local zx strain increment 
c 
c     sig(1)=local x  stress 
c     sig(2)=local y  stress 
c     sig(3)=local z  stress 
c     sig(4)=local xy stress 
c     sig(5)=local yz stress 
c     sig(6)=local zx stress 
c 
c 
c 
c     hsv(1)=1st history variable    
c     hsv(2)=2nd history variable    
c        . 
c        . 
c        . 
c        . 
c     hsv(n)=nth history variable 
c 
c     dt1=current time step size 
c     capa=reduction factor for transverse shear 
c     etype: 
c        eq."brick" for solid elements 
c        eq."shell" for all shell elements 
c        eq."beam"  for all beam elements 
c        eq."dbeam"  for all discrete beam elements 
c 
c     tt=current problem time. 
c 
c     temper=current temperature 
c 
c     es=material tangent modulus 
c 
c 
c 
c 
c 
c 
c 
      include 'nlqparm' 
      character*(*) etype 
      dimension cm(*),eps(*),sig(*),hsv(*),crv(lq1,2,*) 
      dimension es(6,*) 
c 
c     no history variables, NHV=0 
c     deformation gradient stored in hsv(1),...,hsv(9) 
c      
c     compute jacobian 
c      
      detf=hsv(1)*(hsv(5)*hsv(9)-hsv(6)*hsv(8)) 
     1     -hsv(2)*(hsv(4)*hsv(9)-hsv(6)*hsv(7)) 
     2     +hsv(3)*(hsv(4)*hsv(8)-hsv(5)*hsv(7)) 
crv=array representation of curves in keyword deck 
The material tangent modulus is set to 0 prior to entering 
this routine.  It should be expressed in the local system 
upon exiting this routine.  All transformations back to the 
global system is made outside this routine.
APPENDIX A 
c      
c     compute lame parameters 
c      
      xlambda=cm(1)*cm(2)/((1.+cm(2))*(1.-2.*cm(2))) 
      xmu=.5*cm(1)/(1.+cm(2)) 
c      
c     compute tangent stiffness 
c     same for both shells and bricks 
c      
      detfinv=1./detf 
      dmu=xmu-xlambda*log(detf) 
      es(1,1)=detfinv*(xlambda+2.*dmu) 
      es(2,2)=detfinv*(xlambda+2.*dmu)  
      es(3,3)=detfinv*(xlambda+2.*dmu) 
      es(4,4)=detfinv*dmu 
      es(5,5)=detfinv*dmu 
      es(6,6)=detfinv*dmu 
      es(2,1)=detfinv*xlambda 
      es(3,2)=detfinv*xlambda 
      es(3,1)=detfinv*xlambda 
      es(1,2)=es(2,1) 
      es(2,3)=es(3,2) 
      es(1,3)=es(3,1) 
c      
      return 
      end 
User-Defined Materials with Equations of State 
The  following  example  umat44v  is  set  up  to  be  used  with  an  equation  of  state  (EOS).  
Unlike standard models, it updates only the  deviatoric stress and it assigns a value to 
PC, the pressure cut-off.  The pressure cut-off limits the amount of hydrostatic pressure 
that can be carried in tension (i.e., when the pressure is negative).  The default value is 
zero, and a large negative number will allow the material to carry an unlimited pressure 
load  in  tension.    It  is  calculated  within  the  material  model  because  it  is  typically  a 
function  of  the  current  state  of  the  material  and  varies  with  time.    In  this  example, 
however,  it  is  a  constant  value  for  simplicity.    The  pressure  cut-off  array  is  passed 
through  the  named  common  block  eosdloc. 
  Depending  on  the  computing 
environment,  compiler  directives  may  be  required  (e.g.,  the  task  common  directive  in 
the example) for correct SMP execution.  
In addition, the number of history variables, NHV, must be increased by 4 in the input 
file to allocate the extra storage required for the EOS.  The storage is the first 4 variables 
in hsvs, and it must not be altered by the user-defined material model. 
      subroutine umat44v(cm,d1,d2,d3,d4,d5,d6,sig1,sig2, 
     .  sig3,sig4,sig5,sig6,eps,hsvs,lft,llt,dt1siz,capa, 
     .  etype,tt,temps,failels,nlqa,crv) 
      parameter (third=1.0/3.0) 
      include 'nlqparm' 
c 
c***  isotropic plasticity with linear hardening  
c 
c***  updates only the deviatoric stress so that it can be used with 
c     an equation of state 
c 
      character*5 etype
APPENDIX A 
      logical failels 
c 
C_TASKCOMMON (eosdloc) 
      common/eosdloc/pc(nlq) 
c 
      dimension cm(*),d1(*),d2(*),d3(*),d4(*),d5(*),d6(*), 
     & sig1(*),sig2(*),sig3(*),sig4(*),sig5(*),sig6(*), 
     & eps(*),hsvs(nlqa,*),dt1siz(*),temps(*),crv(lq1,2,*), 
     & failels(*) 
c 
c***  shear modulus, initial yield stress, hardening, and pressure cut-off 
      g   =cm(1) 
      sy0 =cm(2) 
      h   =cm(3) 
      pcut=cm(4) 
c 
      ofac=1.0/(3.0*g+h) 
      twog=2.0*g 
c 
      do i=lft,llt 
c 
c***    trial elastic deviatoric stress 
        davg=third*(d1(i)+d2(i)+d3(i)) 
        savg=third*(sig1(i)+sig2(i)+sig3(i)) 
        sig1(i)=sig1(i)-savg+twog*(d1(i)-davg) 
        sig2(i)=sig2(i)-savg+twog*(d2(i)-davg) 
        sig3(i)=sig3(i)-savg+twog*(d3(i)-davg) 
        sig4(i)=sig4(i)+g*d4(i) 
        sig5(i)=sig5(i)+g*d5(i) 
        sig6(i)=sig6(i)+g*d6(i)  
c 
c***    radial return 
        aj2=sqrt(1.5*(sig1(i)**2+sig2(i)**2+sig3(i)**2)+ 
     &           3.0*(sig4(i)**2+sig5(i)**2+sig6(i)**2)) 
        sy=sy0+h*eps(i) 
        eps(i)=eps(i)+ofac*max(0.0,aj2-sy) 
        synew=sy0+h*eps(i) 
        scale=synew/max(synew,aj2) 
c 
c***    scaling for radial return.  note that the stress is now deviatoric. 
        sig1(i)=scale*sig1(i) 
        sig2(i)=scale*sig2(i) 
        sig3(i)=scale*sig3(i) 
        sig4(i)=scale*sig4(i) 
        sig5(i)=scale*sig5(i) 
        sig6(i)=scale*sig6(i) 
c 
c***    set pressure cut-off 
        pc(i)=pcut 
c 
      enddo 
c 
      return 
      end 
Post-processing a user-defined material 
Post-processing a user-defined material is very similar to post-processing a regular LS-
DYNA  material.    There  are  however  some  things  that  are  worth  being  stressed,  all 
dealing with how to post-process history variables.
APPENDIX A 
First, the effective plastic strain is always written to the d3plot database and thus need 
not be requested by the user.  It is in LS-PRE/POST treated just as it is for any other LS-
DYNA material. 
The  number  of  additional  history  variables  written  to  the  d3plot  database  must  be 
requested  as  the  parameter  NEIPH  (for  bricks)  or  NEIPS  (for  shells)  on  *DATABASE_
EXTENT_BINARY.    For  instance,  if  NEIPH  (NEIPS)  equals  2  the  first  two  history 
variables in the history variables array are obtained as history var#1 and history var#2 
in the d3plot database.  By putting NEIPH (NEIPS) equal to NHV, all history variables 
are  written  to  the  d3plot  database.    Furthermore,  if  the  material  uses  the  deformation 
gradient  (IHYPER = 1)  an  additional  9  variables  must  be  requested  to  make  this 
available for post-processing, i.e., put NEIPH (NEIPS) equal to NHV+9.  This makes the 
deformation  gradient  available  in  the  d3plot  database  as  history  variables  NHV+1  to 
NHV+9,  note  however  that  for  shells  it  is  expressed  in  the  co-rotational  system.    If  the 
local coordinate system option (IORTHO = 1) is used, then the deformation gradient is 
expressed in this local system.  To make the deformation gradient in the global system 
for  bricks  and  co-rotational  system  for  shells  available  and  stored  as  history  variables 
NHV+10 to NHV+18, NEIPH (NEIPS) is put equal to NHV+9+9(=NHV+18).
APPENDIX B 
APPENDIX B:  
User Defined Equation of State 
The user can supply his/her own subroutines defining equation of state (EOS) models 
in LS-DYNA.  To invoke a user-defined EOS, one must 
1.  Write a user EOS subroutine that is called by the LS-DYNA user EOS interface. 
2.  Create a custom executable which includes the EOS subroutine. 
3. 
Invoke that subroutine by defining a part in the keyword input deck that uses 
*EOS_USER_DEFINED with the appropriate input parameters. 
Subroutine  ueoslib  and  sample  subroutines  ueos21s  and  ueos21v  are  provided  in  the 
file dyn21b.f.  This text serves as an introductory guide to implementing such a model.  
Note  that  names  of  variables  and  subroutines  below  may  differ  from  the  actual  ones 
depending on platform and current version of LS-DYNA. 
General overview 
When the keyword  *EOS_USER_DEFINED is defined for a part in the keyword deck, LS-
DYNA  calls  the  subroutine  ueoslib  with  the  appropriate  input  data  for  the  EOS 
update.  This subroutine is called twice for each integration point in each element.  The 
first  call  requires  the  EOS  to  calculate  the  bulk  modulus,  and  the  second  updates  the 
pressure and internal energy.  In these routines, which may be modified by the user if 
necessary, the following data structures are initialized for the purpose of being supplied 
to a specific scalar material subroutine. 
iflag –  mode flag 
EQ.-1: for initializing EOS constants 
EQ.0:  for calculating the bulk modulus 
EQ.1:  for the pressure and energy update 
cb –  bulk modulus 
pnew –  the new pressure 
rho0 –  reference density 
hist –  array of user-defined history variables NHV in length 
specen –  internal energy per unit reference volume 
df –  volume ratio, V/V0 
v0 –  the initial volume.   
dvol –  volume increment 
pc –  pressure cut-off
APPENDIX B 
If the vectorization flag is active (IVECT = 1) on the EOS card, variables are, in general, 
stored  in  vector  blocks  of  length  nlq,  with  vector  indices  ranging  from  lft  to  llt  , 
which allows for a more efficient execution of the EOS routine.  As an example, the data 
structures mentioned above for the vectorized case are 
cb(nlq) –  bulk modulus 
pnew(nlq) –  the new pressure  
hist(nlq,*) –  array of user-defined history variables with NHV columns 
specen(nlq) –  internal energy per unit reference volume 
df(nlq) –  volume ratio, V/V0 
v0(nlq) –  the initial volume 
dvol(nlq) –  volume increment 
pc(nlq) –  pressure cut-off 
The value of nlq is set as a parameter in the include file nlqparm, included at the top 
of the subroutine, and varies between machines and operating systems. Each entry in a 
vector  block  is  associated  with  an  element  in  the  finite  element  mesh  for  a  fix 
integration point.  The number of entries in the history variables array (indicated by * 
in  the  above)  matches  the  number  of  history  variables  requested  on  the  material  card 
(NHV).  All history variables are initially zero and are initialized within the EOS on the 
first  time  step,  when  the  logical  variable  first,  passed  through  the  argument  list,  is 
.TRUE.  Furthermore,  all  user-defined  EOS  models  require  a  bulk  modulus,  cb,  for 
transmitting  boundaries,  contact  interfaces,  rigid  body  constraints,  and  time  step 
calculations.    In  addition  to  the  variables  mentioned  above,  the  following  data  can  be 
supplied  to  the  user  material  routines,  regardless  of  whether  vectorization  is  used  or 
not. 
eosp(*) –  array of material constants from the input file 
tt –  current time 
crv(lq1,2,*) –  array representation of curves defined in the keyword deck. 
A  user  defined  EOS  subroutine,  ueosXXs  in  the  scalar  case  or  ueosXXv  in  the  vector 
case, will be called for parts that point to *EOS_USER_DEFINED in the input deck.  The 
letters XX stand for a number between 21 and 30 that matches the input variable EOST 
in  the    *EOS_USER_DEFINED  keyword.    During  the  initialization  phase,  the  EOS  is 
called with iflag = -1 to permit the initialization of constants in the user EOS.  Although 
fewer than 48 constants may be read into the array eosp during the input, the user may 
use all 48 within the EOS subroutines.  The user defined subroutine should calculate the 
bulk  modulus  when  iflag = 0,  and  update  the  pressure,  internal  energy  and  history 
variables when iflag = 1. 
The use of curves (*DEFINE_CURVE) is discussed in Appendix A. 
A  sample  scalar  user  subroutine  for  a  Gruneisen  EOS  is  provided  below  and  it  is 
immediately followed by its vector counterpart.
APPENDIX B 
Sample user subroutine 21 
      subroutine ueos21s(iflag,cb,pnew,hist,rho0,eosp,specen, 
     &                   df,dvol,v0,pc,dt,tt,crv,nnpcrv,first) 
      include 'nlqparm' 
c 
c***  example scalar user implementation of the Gruneisen EOS 
c 
c***  variables 
c          iflag ----- =0 calculate bulk modulus 
c                      =1 update pressure and energy 
c          cb -------- bulk modulus  
c          pnew ------ new pressure 
c          hist ------ history variables 
c          rho0 ------ reference density 
c          eosp ------ EOS constants 
c          specen ---- energy/reference volume 
c          df -------- volume ratio, v/v0 = rho0/rho 
c          dvol ------ change in volume over time step 
c          v0 -------- reference volume 
c          pc -------- pressure cut-off 
c          dt -------- time step size 
c          tt -------- current time 
c          crv ------- curve array 
c          nnpcrv ---- number of points in each curve 
c          first ----- logical .true.  for tt,crv,first time step 
c                      (for initialization of the history variables) 
c 
      logical first 
c 
      dimension hist(*),eosp(*),crv(lq1,2,*) 
      integer nnpcrv(*) 
c 
      c  =eosp(1) 
      s1 =eosp(2) 
      s2 =eosp(3) 
      s3 =eosp(4) 
      g0 =eosp(5) 
      sa =eosp(6) 
      s11=s1-1. 
      s22=2.*s2 
      s33=3.*s3 
      s32=2.*s3 
      sad2=.5*sa 
      g0d2=1.-.5*g0 
      roc2=rho0*c**2 
c 
c***  calculate the bulk modulus for the EOS contribution to the sound speed 
      if (iflag.eq.0) then 
        xmu=1.0/df-1. 
        dfmu=df*xmu 
        facp=.5*(1.+sign(1.,xmu)) 
        facn=1.-facp 
        xnum=1.+xmu*(+g0d2-sad2*xmu) 
        xdem=1.-xmu*(s11+dfmu*(s2+s3*dfmu)) 
        tmp=facp/(xdem*xdem) 
        a=roc2*xmu*(facn+tmp*xnum) 
        b=g0+sa*xmu 
        pnum=roc2*(facn+facp*(xnum+xmu*(g0d2-sa*xmu))) 
        pden=2.*xdem*(-s11 +dfmu*(-s22+dfmu*(s2-s33+s32*dfmu))) 
        cb=pnum*(facn+tmp)-tmp*a*pden+sa*specen+ 
     &        b*df**2*max(pc,(a+b*specen)) 
c 
c***  update the pressure and internal energy 
      else 
        xmu=1.0/df-1.
APPENDIX B 
        dfmu=df*xmu 
        facp=.5*(1.+sign(1.,xmu)) 
        facn=1.-facp 
        xnum=1.+xmu*(+g0d2-sad2*xmu) 
        xdem=1.-xmu*(s11+dfmu*(s2+s3*dfmu)) 
        tmp=facp/(xdem*xdem) 
        a=roc2*xmu*(facn+tmp*xnum) 
        b=g0+sa*xmu 
        dvov0=0.5*dvol/v0 
        denom=1.+ b*dvov0                                      
        pnew=(a+specen*b)/max(1.e-6,denom)                    
        pnew=max(pnew,pc) 
        specen=specen-pnew*dvov0 
      endif 
c 
      return 
      end 
      subroutine ueos21v(lft,llt,iflag,cb,pnew,hist,rho0,eosp,specen, 
     &                   df,dvol,v0,pc,dt,tt,crv,nnpcrv,first) 
      include 'nlqparm' 
c 
c***  example vectorized user implementation of the Gruneisen EOS 
c 
c***  variables 
c          lft,llt --- tt,crv,first and last indices into arrays 
c          iflag ----- =0 calculate bulk modulus 
c                      =1 update pressure and energy 
c          cb -------- bulk modulus  
c          pnew ------ new pressure 
c          hist ------ history variables 
c          rho0 ------ reference density 
c          eosp ------ EOS constants 
c          specen ---- energy/reference volume 
c          df -------- volume ratio, v/v0 = rho0/rho 
c          dvol ------ change in volume over time step 
c          v0 -------- reference volume 
c          pc -------- pressure cut-off 
c          dt -------- time step size 
c          tt -------- current time 
c          crv ------- curve array 
c          nnpcrv ---- number of points in each curve 
c          first ----- logical .true.  for tt,crv,first time step 
c                      (for initialization of the history variables) 
c 
      logical first 
c 
      dimension cb(*),pnew(*),hist(nlq,*),eosp(*), 
     &          specen(*),df(*),dvol(*),pc(*),v0(*) 
      dimension crv(lq1,2,*) 
      integer nnpcrv(*) 
c 
      c  =eosp(1) 
      s1 =eosp(2) 
      s2 =eosp(3) 
      s3 =eosp(4) 
      g0 =eosp(5) 
      sa =eosp(6) 
      s11=s1-1. 
      s22=2.*s2 
      s33=3.*s3 
      s32=2.*s3 
      sad2=.5*sa 
      g0d2=1.-.5*g0 
      roc2=rho0*c**2 
c 
c***  calculate the bulk modulus for the EOS contribution to the sound speed
APPENDIX B 
      if (iflag.eq.0) then 
        do i=lft,llt 
          xmu=1.0/df(i)-1. 
          dfmu=df(i)*xmu 
          facp=.5*(1.+sign(1.,xmu)) 
          facn=1.-facp 
          xnum=1.+xmu*(+g0d2-sad2*xmu) 
          xdem=1.-xmu*(s11+dfmu*(s2+s3*dfmu)) 
          tmp=facp/(xdem*xdem) 
          a=roc2*xmu*(facn+tmp*xnum) 
          b=g0+sa*xmu 
          pnum=roc2*(facn+facp*(xnum+xmu*(g0d2-sa*xmu))) 
          pden=2.*xdem*(-s11 +dfmu*(-s22+dfmu*(s2-s33+s32*dfmu))) 
          cb(i)=pnum*(facn+tmp)-tmp*a*pden+sa*specen(i)+ 
     &          b*df(i)**2*max(pc(i),(a+b*specen(i))) 
        enddo 
c 
c***  update the pressure and internal energy 
      else 
        do i=lft,llt 
          xmu=1.0/df(i)-1. 
          dfmu=df(i)*xmu 
          facp=.5*(1.+sign(1.,xmu)) 
          facn=1.-facp 
          xnum=1.+xmu*(+g0d2-sad2*xmu) 
          xdem=1.-xmu*(s11+dfmu*(s2+s3*dfmu)) 
          tmp=facp/(xdem*xdem) 
          a=roc2*xmu*(facn+tmp*xnum) 
          b=g0+sa*xmu 
          dvov0=0.5*dvol(i)/v0(i) 
          denom=1.+b*dvov0                                      
          pnew(i)=(a+specen(i)*b)/max(1.e-6,denom)                    
          pnew(i)=max(pnew(i),pc(i)) 
          specen(i)=specen(i)-pnew(i)*dvov0 
        enddo 
      endif 
c 
      return 
      end 
The  Gruneisen  EOS  implemented  in  the  example  subroutines  has  the  same  form  as 
*EOS_GRUNEISEN, EOS Form 4.  Its update of the pressure and the internal energy are 
typical for an EOS that is linear in the internal energy, 
𝑃 = 𝐴(𝜌) + 𝐵(𝜌)𝐸 
where  A and B correspond to the variables a and b in the example subroutines, and E is 
specen.  Integrating the energy equation with the trapezoidal rule gives 
𝐸𝑛+1 = 𝐸𝑛 +
(𝜎 ′𝑛 + 𝜎 ′𝑛+1 )Δ𝜀 −
(𝑃𝑛 + 𝑞𝑛 + 𝑃𝑛+1 + 𝑞𝑛+1 )
Δ𝑉
𝑉0
where the superscripts refer to the time step, Δ𝑉 is the change in the volume associated 
with  the  Gauss  point  and  V0  is  the  reference  volume.    Collecting  all  the  energy 
contributions on the right hand side except for the contribution from the new pressure 
gives a simple linear relationship between the new internal energy and pressure, 
𝐸𝑛+1 = 𝐸̃ −
𝑃𝑛+1Δ𝑉
2𝑉0
.
APPENDIX B 
The  value  of  specen  passed  to  ueosXX  for  the  pressure  and  energy  update 
corresponds  to𝐸̃.  Substituting  this  relation  into  the  EOS  and  solving  for  the  new 
pressure gives 
𝑃𝑛+1 =
𝐴𝜌𝑛+1 + 𝐵𝜌𝑛+1𝐸̃
1 + 𝐵Δ𝑉
2𝑉0
. 
The  final  update  of  the  new  energy  is  calculated  using  the  new  pressure.    For  a  more 
general EOS, the nonlinear equation in the new pressure, 
𝑃𝑛+1 = 𝑃 (𝜌𝑛+1, 𝐸̃ −
𝑃𝑛+1Δ𝑉
2𝑉0
) 
is solved iteratively using Newton iteration or successive substitution. 
The pressure cut-off, pc, is used to limited the amount of pressure that can be generated 
by  tensile  loading,  pnew=max(pnew,pc).    Its  value  is  usually  specified  in  the  *MAT 
input, e.g., *MAT_JOHNSON_COOK.  It is not enforced outside of the EOS subroutines, 
and  it  is  up  to  the  user  to  determine  whether  or  not  to  enforce  the  pressure  cut-off  in 
ueosXX.    If  the  user  does  enforce  it,  the  pressure  cut-off  should  be  applied  before  the 
final update to the internal energy otherwise the energy will be incorrect. 
Many of the calculations performed to calculate the bulk modulus are the same as those 
for  updating  the  pressure  and  energy.    Since  the  bulk  modulus  calculation  always 
precedes  the  pressure  update,  the  values  may  be  saved  in  a  common  block  during  the 
bulk modulus calculation to reduce the cost of the pressure update.  The arrays used to 
store the values in the vectorized subroutines should be dimensioned by nlq. 
One  of  the  most  common  errors  in  implementing  an  EOS  from  a  paper  or  book  is  the 
use of the wrong internal energy.  There are three internal energies in common use: the 
energy per unit mass,𝑒𝑀, the energy per unit current volume,𝑒𝑉, and the energy per unit 
reference  volume,  E.    LS-DYNA  always  uses  the  energy  per  unit  reference  volume.  
Some useful relations for converting between EOS in the literature and the variables in 
LS-DYNA are 
𝑒𝑉 = 𝐸
𝑒𝑀 = 𝐸
=
=
𝑉0
𝑉0
𝑉0
specen
df
specen
rho0
rho0
df
𝜌 = 𝜌0
=
APPENDIX C 
APPENDIX C:  User Defined Element 
Interface for Solids and Shells 
In  this  appendix  the  user-defined  element  interface  for  solids  and  shells  is  described.  
The  interface  can  accommodate  either  an  integrated  or  a  resultant  element.    For  the 
integrated  element,  the  user  needs  to  supply  two  matrices  defining  the  kinematical 
properties  of  the  element,  and  choose  between  using  standard  LS-DYNA  hourglass 
stabilization,  a  user-defined  stabilization,  or  no  stabilization  when  zero  energy  modes 
are  not  present.    The  number  and  location  of  the  integration  points  is  arbitrary,  i.e., 
user-defined.    For  the  resultant/discrete  element  formulations,  the  force  and  stiffness 
assembly must also be implemented.  History variables can be associated with the user 
defined elements.  If desired, the element may utilize more than the conventional 3 (for 
bricks) and 6 (for shells) degrees-of-freedom per node. 
The user element is implemented according to how standard elements are implemented 
in  LS-DYNA  with  the  exception  that  two  user  routines  are  called  for  setting  up  the 
matrices  of  interest.    In  the  end,  the  gradient-displacement  matrix  𝐵𝑖𝑗𝑘𝐾  is  constructed 
with the property that 
𝐵𝑖𝑗𝑘𝐾𝑢𝑘𝐾 =
∂𝑣𝑖
∂𝑥𝑗
where 𝑢𝑘𝐾 is the vector of velocity nodal degrees of freedom and the right hand side is 
the velocity gradient.  Moreover, the determinant 𝐽 of the jacobian matrix determining 
the  mapping  from  the  isoparametric  to  physical  domain  is  needed  for  numerical 
integration.  From these expressions, the strains are determined as the symmetric part of 
the  velocity  gradient  and  the  spin  as  the  corresponding  antisymmetric  part.    The 
stresses are evaluated using the constitutive models in LS-DYNA and the internal forces 
are obtained from 
𝑓𝑘𝐾 = ∫ 𝜎𝑖𝑗𝐵𝑖𝑗𝑘𝐾𝑑𝑉 
where 𝜎𝑖𝑗 are the stresses.  Furthermore, the geometric and material tangent stiffnesses 
are obtained through 
and 
𝐾𝑖𝐼𝑗𝐽
mat = ∫ 𝐶𝑘𝑙𝑚𝑛𝐵𝑘𝑙𝑖𝐼𝐵𝑚𝑛𝑗𝐽𝑑𝑉 
geo = ∫ 𝜎𝑚𝑛𝐵𝑘𝑚𝑖𝐼𝐵𝑘𝑛𝑗𝐽𝑑𝑉 
𝐾𝑖𝐼𝑗𝐽
where 𝐶𝑘𝑙𝑚𝑛 is the tangent modulus for the material.  The integrals are evaluated using 
user-defined quadrature using the determinant 𝐽.
APPENDIX C 
For  user-defined  hourglass  control,  the  user  must  provide  the  corresponding  internal 
force  and  stiffness  contribution  in  a  separate  user  routine.    There  is  also  the  option  to 
provide the force and stiffness matrix directly for the entire element. 
To invoke a user-defined element one must do the following: 
1.  Write  user  element  subroutine  that  defines  the  kinematics  or  kinetics  of  the 
element. 
2.  Create a custom executable which includes these subroutines. 
3. 
Invoke the element by specifying this on the corresponding *SECTION card. 
The  dummy  subroutines  for  the  user  defined  elements  are  provided  to  the  user  in  a 
FORTRAN source file for you to modify along with the necessary object files to compile 
a new executable.  Contact LSTC or your local distributor for information about how to 
obtain  these  files  as  well  as  what  compiler/version  to  use  for  your  specific  platform.  
Up to five user elements can simultaneously be used for bricks and shells (i.e.  a total of 
ten).  This text serves as an introductory guide on how to implement such an element. 
General overview 
To activate a user-defined element, it is necessary to set ELFORM to a number between 
101 and 105 on the *SECTION definition.  By doing so, the kinematics of the elements 
in the corresponding part will be determined from calling the subroutine 
subroutine uXXX_bYYY(bmtrx,gmtrx,gjac,... 
⋮ 
dimension bmtrx(nlq,3,3,*),gmtrx(nlq,3,3),gjac(*) 
where XXX is substituted for shl for a shell-section and sld for a solid-section and YYY 
is  the  number  specified  in  position  ELFORM.    Depending  on  the  choice  of  ITAJ  in  the 
input, the user should set the matrices as follows. 
If ITAJ = 0, then set the isoparametric gradient-displacement matrix, represented by 
the array bmtrx , and jacobian matrix, represented by the array gmtrx.  Here, the first 
index corresponds to the LS-DYNA block loop index where nlq is the block size.  For a 
more  convenient  notation  in  the  following,  we  assign  a  correspondence  between  the 
arrays gmtrx and bmtrx in the subroutines to matrices/tensors as follows 
gmtrx(*,i,j) -  𝑔𝑖𝑗 
bmtrx(*,i,j,k) -  𝑏𝑖𝑗𝑘 
These matrices should be determined so that at the current integration point:
APPENDIX C 
𝑔𝑖𝑗 =
𝑏𝑖𝑗𝑘𝑢𝑘 =
∂𝑥𝑖
∂𝜉𝑗
∂𝑣𝑖
∂𝜉𝑗
Δ𝑡 
In  the  above,  summation  over  repeated  indices  is  assumed.    We  use  the  following 
notation: 
𝑥𝑖(𝜉1, 𝜉2, 𝜉3, 𝑡) =  ith  component  of  the  current  position  vector  at  the 
isoparametric coordinate (𝜉1, 𝜉2, 𝜉3) and time t. 
𝑣𝑖(𝜉1, 𝜉2, 𝜉3, 𝑡) =  ith  component  of  the  velocity  vector  at  the  isoparemetric 
coordinate (𝜉1, 𝜉2, 𝜉3) and time t. 
Δ𝑡 =  current time step 
𝑢𝑘 =  kth component of generalized local displacements 
𝜉𝑖 =  ith component of the isoparametric coordinate ranging from -
1.0 to 1.0 
For shells, there is an option to get all variables in either the LS-DYNA local coordinate 
system  (ILOC=0)  or  in  the  global  coordinate  system  (ILOC=1).    The  matrix  for  the 
coordinate system transformation is also passed to the user routines where the columns 
represent the local unit base vectors.  The resulting strains must always be in the local 
coordinate system for the constitutive evaluations.  For no extra degrees of freedom , the index 𝑘 in the displacement expression is determined from the formula 
𝑘 = 𝑛(𝑚 − 1) + 𝑑 
where 𝑛 = 3 if only translational degrees of freedom are present (typical for solids) and 
𝑛 = 6 if rotational degrees of freedom are present (typical for shells), 𝑚 is the local node 
number  (𝑚 = 1,2, . ..)  and  𝑑  is  the  degree  of  freedom.    The  translational  degrees  of 
freedom correspond to 𝑑 ≤ 3 and the rotational degrees of freedom to 4 ≤ 𝑑 ≤ 6. 
If  ITAJ=1,  the  user  should  set  up  the  physical  gradient-displacement  matrix, 
represented  by  the  array  bmtrx,  and  jacobian  determinant,  represented  by  the  array 
gjac.  Again, we assign a correspondence between the arrays gjac and bmtrx in the 
subroutines to matrices/tensors as follows 
gjac(*) -  𝐽 
bmtrx(*,i,j,k) -  𝑏𝑖𝑗𝑘 
These matrices should be determined so that at the current integration point: 
𝐽 = det
∂𝑥𝑖
∂𝜉𝑗
APPENDIX C 
𝑏𝑖𝑗𝑘𝑢𝑘 =
∂𝑣𝑖
∂𝑥𝑗
Δ𝑡 
To be able to set up these matrices, a set of additional auxiliary variables are passed to 
the user element subroutines.  These include the isoparametric coordinate, the element 
thickness,  and  the  shape  function  values,  and  derivatives.    Again,  for  shells  these  are 
expressed in either the local or global coordinate system depending on the user’s choice.  
For  more  information  on  these  variables,  the  user  is  referred  to  the  comments  in  the 
subroutines. 
The integrated elements can use up to a total of 100 integration points (in the plane for 
shells)  at  arbitrary  locations.    These  must  be  specified  in  terms  of  isoparametric 
coordinates and weights following the first of the user-defined cards in the *SECTION_
…  input.    The  isoparametric  coordinates  should  range  from  –1  to  1  and  the  weights 
should sum up to 4 for shells and 8 for solids. 
It  may  be  necessary  to  incorporate  hourglass  stabilization  to  suppress  zero  energy 
modes,  this  is  done  by  putting  IHGF.GT.0  in  the  input.    For  IHGF.EQ.1,  the  LS-
DYNA  hourglass  routines  are  used  automatically  and  for  IHGF.EQ.2  or  IHGF.EQ.3 
the user must provide hourglass force and stiffness in a specific user-defined routine.  If 
IHGF.EQ.3,  physical  stabilization  becomes  available  since  the  resultant  material 
tangent  moduli  are  passed  to  the  hourglass  routine  to  provide  the  current  membrane, 
bending  and  coupled  membrane-bending  stiffness  of  the  material.    With  𝐶𝑖𝑗  denoting 
the  material  tangent  modulus  in  matrix  form,  the  resultant  tangent  moduli  are 
expressed as 
(membrane)
𝐶̅
0 = ∫ 𝐶𝑖𝑗 𝑑𝑉
𝑖𝑗
𝐶̅
1 = ∫ 𝑧1𝐶𝑖𝑗 𝑑𝑉 (membrane − bending)
𝑖𝑗
𝐶̅
2 = ∫ 𝑧2𝐶𝑖𝑗 𝑑𝑉 (bending)
𝑖𝑗
where  𝑧  is  the  thickness  coordinate  for  shells.    For  solids,  only  the  first  resultant 
modulus  is  passed.    In  this  case  the  array  has  21  entries  that  correspond  to  the 
subdiagonal  terms  of  the  6  by  6  resultant  matrix.    For  the  matrix  index  (𝑖, 𝑗)  in  the 
material  tangent  modulus  matrix,  where  𝑖 ≥ 𝑗,  the  index  𝐼  of  the  array  passed  to  the 
routine is given by 
𝐼 = 𝑖(𝑖 − 1)/2 + 𝑗 
i.e., the subdiagonal terms are stored row-wise in the array.  For shells, all three moduli 
are passed in the local coordinate system where each array has 15 entries corresponding 
to  the  subdiagonal  terms  of  the  5  by  5  resultant  matrices.    The  through  thickness 
direction is here eliminated from the plane stress assumption.  The formula for the array 
indices transformation above holds.  This subroutine is called 
subroutine uXXX_eYYY(force,stiff,ndtot,... 
⋮
APPENDIX C 
dimension force(nlq,*),stiff(nlq,ndtot,*) 
where again XXX and YYY should be substituted as described for the other subroutines 
in the above.  The variables in the subroutine corresponds to the force and stiffness as 
force(*,i) -  𝑓𝑖 
stiff(*,i,j) -  𝐾𝑖𝑗 
where  the  indices  corresponds  to  node  and degree  of  freedom  numbers  exactly  as  for 
the displacements.  For shells the force and stiffness is set up in the local element system 
(ILOC=0)  or  global  system  (ILOC=1).    The  variable  ndtot  is  the  total  number  of 
degrees  of  freedom  for  the  element.    Passed  to  this  subroutine  are  also  the  property 
parameters  and  history  variables  associated  with  the  element.    The  values  of  the 
property parameters are defined in the input of a user-defined element.  No more than 
40  property  parameters  and  100  history  variables  can  be  used  for  each  user-defined 
element.  The history variables must be updated in this routine by the user. 
Resultant/discrete elements 
By putting NIP(P) equal to 0 in the input, a resultant/discrete element is assumed.  For 
this  option  (which  is  incompatible  with  IHGF.GT.0)  the  user  must  provide  force  and 
stiffness  in  the  same  user-defined  routine  as  for  the  user-defined  hourglass  control.  
This  means  that  no  material  routine  is  called  to  update  stresses  and  history  variables, 
rather  stresses  and  history  variables  are  to  be  updated  from  within  the  user  element 
routine. 
Nevertheless,  the  user  should  define  *MAT_ELASTIC  as  the  material  for  the 
corresponding  part  with  suitable  values  of  the  Young’s  modulus  and  Poisson’s  ratio.  
These  material  properties  are  used  to  calculate  the  time  step  and  for  determining 
contact stiffnesses.  Again, property parameters and history variables are passed to the 
routine,  and  for  shells  also  the  thicknesses  of  the  elements.    For  the  shell  thickness 
update option (ISTUPD.GT.0 on *CONTROL_SHELL) it is up to the user to update the 
thicknesses  in  this  routine.    For  this  option,  and  this  option  only,  the  stiffness  matrix 
assembled  in  the  element  routines  can  be  input  as  nonsymmetric  if  LCPACK=3  on 
*CONTROL_IMPLICIT_SOLVER, i.e., if the nonsymmetric solver is used to update the 
Newton iterates. 
In what follows, a short description of the additional features associated with the user 
elements is given. 
Nodal fiber vectors 
If  a  user-defined  shell  element  formulation  uses  the  nodal  fiber  vectors,  this  must  be 
specified by putting IUNF=1 on the *SECTION_SHELL card.  With this option the nodal
APPENDIX C 
fiber  vectors  are  processed  in  the  element  routines  and  can  be  used  as  input  for 
determining the 𝑏𝑖𝑗𝑘, 𝑔𝑖𝑗/𝐽, 𝑓𝑖  and 𝐾𝑖𝑗 tensors/matrices in the user routines.  If not, it is 
assumed that the fiber direction is normal to the plane of the shell at all times.  These 
are expressed in either the local or global system depending on the user’s choice.  See 
comments in the subroutines for more information. 
Extra degrees of freedom 
Exotic element formulations may require extra degrees-of-freedom per node besides the 
translational  (and  rotational)  degrees-of-freedom.    Currently,  up  to  3  extra  degrees  of 
freedom  per  node  can  be  used  for  user-defined  elements.    To  use  extra  degrees  of 
freedom, a scalar node must be defined for each node that makes up the connectivity of 
the user element.  A scalar node is defined using the keyword *NODE_SCALAR_VALUE, 
in  which  the  user  also  prescribe  initial  and  boundary  conditions  associated  with  the 
extra variables.  The connectivity of the user elements must then be specified with the 
option *ELEMENT_SOLID_DOF or *ELEMENT_SHELL_DOF, where an extra line is used 
to connect the scalar nodes to the element.  As an example: 
*NODE_SCALAR_VALUE 
$    NID              V1              V2              V3     NDF 
      11             1.0                                       1 
      12             1.0                                       1 
      13             1.0                                       1 
      14             1.0                                       1 
*ELEMENT_SHELL_DOF 
$    EID     PID      N1      N2      N3      N4 
       1       1       1       2       3       4 
$                    NS1     NS2     NS3     NS4 
                      11      12      13      14 
defines  an  element  with  one  extra  degree  of  freedom.    The  initial  value  of  the 
corresponding  variable  is  1.0  and  it  is  unconstrained.    Finally,  the  user  sets  the 
parameter NXDOF on the *SECTION_… card to 1, 2 or 3 depending on how many extra 
degrees  of  freedom  that  should  be  used  in  the  user-defined  element.    An  array  xdof 
containing the current values of these extra variables are passed to the user routines for 
setting  up  the  correct  kinematical  properties,  see  comments  in  the  routines  for  more 
information.  The formula for the displacement index changes to 
𝑘 = (𝑛 + 𝑛𝑥𝑑𝑜𝑓 )(𝑚 − 1) + 𝑑 
where 𝑛𝑥𝑑𝑜𝑓   is  the  number  of  extra  degrees  of  freedom.    The  extra  degrees  of  freedom 
for each node corresponds to 𝑛 + 1 ≤ 𝑑 ≤ 𝑛 + 𝑛𝑥𝑑𝑜𝑓 . For dynamic simulations, the mass 
corresponding  to  these  extra  nodes  are  defined  using  *ELEMENT_INERTIA  or 
*ELEMENT_MASS.
APPENDIX C 
Related keywords: 
The following is a list of keywords that apply to the user defined elements 
The *SECTION_SHELL card 
A  third  card  with  accompanying  optional  cards  of  the  *SECTION_SHELL  keyword 
must be added if the user defined element option is invoked 
Additional Card for ELFORM = 101,102,103,104 or 105 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NIPP 
NXDOF 
IUNF 
IHGF 
ITAJ 
LMC 
NHSV 
ILOC 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
Include NIPP cards according to the following format.  
  Card 4 
Variable 
Type 
1 
XI 
F 
2 
3 
4 
5 
6 
7 
8 
ETA 
WGT 
F 
F 
Define LMC property parameters using 8 parameters per card.  
  Card 5 
Variable 
1 
P1 
Type 
F 
2 
P2 
F 
3 
P3 
F 
4 
P4 
F 
5 
P5 
F 
6 
P6 
F 
7 
P7 
F 
8 
P8 
F 
  VARIABLE   
ELFORM 
DESCRIPTION
GT.100.AND.LT.106: User-defined shell 
NIPP 
Number of in-plane integration points for user-defined shell (0 if 
resultant element)
APPENDIX C 
  VARIABLE   
NXDOF 
DESCRIPTION
Number  of  extra  degrees  of  freedom  per  node  for  user-defined 
shell 
IUNF 
Flag for using nodal fiber vectors in user-defined shell 
EQ.0: Nodal fiber vectors are not used . 
EQ.1: Nodal fiber vectors are used 
IHGF 
Flag for using hourglass stabilization (NIPP.GT.0) 
EQ.0: Hourglass stabilization is not used 
EQ.1: LS-DYNA hourglass stabilization is used 
EQ.2: User-defined hourglass stabilization is used 
EQ.3: Same as 2, but the resultant material tangent moduli are
passed 
ITAJ 
Flag for setting up finite element matrices (NIPP.GT.0) 
EQ.0: Set up matrices wrt isoparametric domain 
EQ.1: Set up matrices wrt physical domain 
LMC 
Number of property parameters 
NHSV 
Number of history variables 
ILOC 
Local coordinate system option 
EQ.0: All variables are passed in the local element system   
EQ.1: All variables are passed in the global system 
XI 
ETA 
WGT 
PI 
First isoparametric coordinate 
Second isoparametric coordinate 
Isoparametric weight 
Ith property parameter 
For more information on the variables the user may consult the previous sections in this 
appendix.
APPENDIX C 
The *SECTION_SOLID card 
A  second  card  with  accompanying  optional  cards  of  the  *SECTION_SOLID  keyword 
must be added if the user defined elements option is invoked. 
Additional card for ELFORM = 101,102,103,104 or 105 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NIP 
NXDOF 
IHGF 
ITAJ 
LMC 
NHSV 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
Include NIP cards according to the following format.  
  Card 4 
Variable 
Type 
1 
XI 
F 
2 
3 
4 
5 
6 
7 
8 
ETA 
ZETA 
WGT 
F 
F 
F 
Define LMC property parameters using 8 parameters per card.  
  Card 5 
Variable 
1 
P1 
Type 
F 
2 
P2 
F 
3 
P3 
F 
4 
P4 
F 
5 
P5 
F 
6 
P6 
F 
7 
P7 
F 
8 
P8 
F 
  VARIABLE   
ELFORM 
NIP 
NXDOF 
DESCRIPTION
GT.100.AND.LT.106: User-defined solid 
Number of integration points for user-defined solid (0 if resultant 
element) 
Number  of  extra  degrees  of  freedom  per  node  for  user-defined 
solid
APPENDIX C 
  VARIABLE   
DESCRIPTION
IHGF 
Flag for using hourglass stabilization (NIP.GT.0) 
EQ.0: Hourglass stabilization is not used 
EQ.1: LS-DYNA hourglass stabilization is used 
EQ.2: User-defined hourglass stabilization is used 
EQ.3: Same as 2, but the resultant material tangent moduli are
passed 
ITAJ 
Flag for setting up finite element matrices (NIP.GT.0) 
EQ.0: Set up matrices wrt isoparametric domain 
EQ.1: Set up matrices wrt physical domain 
LMC 
Number of property parameters 
NHSV 
Number of history variables 
XI 
ETA 
ZETA 
WGT 
First isoparametric coordinate 
Second isoparametric coordinate 
Third isoparametric coordinate 
Isoparametric weight 
PI 
Ith property parameter 
For more information on the variables the user may consult the previous sections in this 
appendix. 
Sample User Shell Element 101 (Belytschko-Tsay shell) 
The geometry of the Belytschko-Tsay element in local coordinates can be written 
𝑥𝑖 = (𝑥𝑖𝐼 +
𝑣𝑖 = (𝑣𝑖𝐼 +
𝜉3𝛿𝑖3)𝑁𝐼(𝜉1, 𝜉2) 
𝜉3𝑒𝑖𝑗3𝜔𝑗𝐼)𝑁𝐼(𝜉1, 𝜉2) 
Where, 
𝑥𝑖𝐼 = 𝑖th component of coordinate of node𝐼 
𝑣𝑖𝐼 = 𝑖th component of translational velocity of node 𝐼 
𝜔𝑗𝐼 = 𝑗th component of rotational velocity of node 𝐼
APPENDIX C 
𝑡 = thickness of element 
𝑒𝑖𝑗𝑘 = permutation tensor 
𝑁𝐼 = shape function localized at node 𝐼 
𝛿𝑖3 = Kronecker delta 
Taking the derivative of these expressions with respect to the isoparametric coordinate 
yields 
and 
𝜉3𝛿𝑖3)
𝜉3𝛿𝑖3)
∂𝑁𝐼
∂𝜉1
∂𝑁𝐼
∂𝜉2
∂𝑥𝑖
∂𝜉1
∂𝑥𝑖
∂𝜉2
∂𝑥𝑖
∂𝜉3
= (𝑥𝑖𝐼 +
= (𝑥𝑖𝐼 +
=
𝛿𝑖3 
∂𝑣𝑖
∂𝜉1
∂𝑣𝑖
∂𝜉2
∂𝑣𝑖
∂𝜉3
= (𝑣𝑖𝐼 +
= (𝑣𝑖𝐼 +
𝜉3𝑒𝑖𝑗3𝜔𝑗𝐼)
𝜉3𝑒𝑖𝑗3𝜔𝑗𝐼)
∂𝑁𝐼
∂𝜉1
∂𝑁𝐼
∂𝜉2
=
𝑒𝑖𝑗3𝜔𝑗𝐼𝑁𝐼 
respectively.    Using  these  expressions  the  element  is  implemented  as  a  user-defined 
shell as follows. 
      subroutine ushl_b101(bmtrx,gmtrx,gjac, 
     1     xi,eta,zeta, 
     2     n1,n2,n3,n4, 
     3     dn1dxi,dn2dxi,dn3dxi,dn4dxi, 
     4     dn1deta,dn2deta,dn3deta,dn4deta, 
     5     x1,x2,x3,x4,y1,y2,y3,y4,z1,z2,z3,z4, 
     6     xdof, 
     7     thick,thck1,thck2,thck3,thck4, 
     8     fx1,fx2,fx3,fx4, 
     9     fy1,fy2,fy3,fy4, 
     .     fz1,fz2,fz3,fz4, 
.     gl11,gl21,gl31,gl12,gl22,gl32,gl13,gl23,gl33, 
     .     lft,llt) 
      include 'nlqparm' 
c 
c     Compute b and g matrix for user-defined shell 101 
c 
      dimension bmtrx(nlq,3,3,*),gmtrx(nlq,3,3),gjac(nlq) 
      REAL n1,n2,n3,n4 
      dimension x1(nlq),x2(nlq),x3(nlq),x4(nlq) 
      dimension y1(nlq),y2(nlq),y3(nlq),y4(nlq) 
      dimension z1(nlq),z2(nlq),z3(nlq),z4(nlq)
APPENDIX C 
      dimension thick(nlq) 
      dimension thck1(nlq),thck2(nlq),thck3(nlq),thck4(nlq) 
      dimension xdof(nlq,8,3) 
      dimension fx1(nlq),fx2(nlq),fx3(nlq),fx4(nlq) 
      dimension fy1(nlq),fy2(nlq),fy3(nlq),fy4(nlq) 
      dimension fz1(nlq),fz2(nlq),fz3(nlq),fz4(nlq) 
 dimension gl11(nlq),gl21(nlq),gl31(nlq), 
.      gl12(nlq),gl22(nlq),gl32(nlq), 
.      gl13(nlq),gl23(nlq),gl33(nlq)   
c 
      do i=lft,llt 
c 
         gmtrx(i,1,1)= 
     1        x1(i)*dn1dxi+x2(i)*dn2dxi+ 
     2        x3(i)*dn3dxi+x4(i)*dn4dxi 
         gmtrx(i,2,1)= 
     1        y1(i)*dn1dxi+y2(i)*dn2dxi+ 
     2        y3(i)*dn3dxi+y4(i)*dn4dxi 
         gmtrx(i,3,1)= 
     1        0. 
         gmtrx(i,1,2)= 
     1        x1(i)*dn1deta+x2(i)*dn2deta+ 
     2        x3(i)*dn3deta+x4(i)*dn4deta 
         gmtrx(i,2,2)= 
     1        y1(i)*dn1deta+y2(i)*dn2deta+ 
     2        y3(i)*dn3deta+y4(i)*dn4deta 
         gmtrx(i,3,2)= 
     1        0. 
         gmtrx(i,1,3)= 
     1        0. 
         gmtrx(i,2,3)= 
     1        0. 
         gmtrx(i,3,3)= 
     1        .5*thick(i) 
c 
         coef=.5*thick(i)*zeta 
c 
         bmtrx(i,1,1,1) =dn1dxi 
         bmtrx(i,1,1,7) =dn2dxi 
         bmtrx(i,1,1,13)=dn3dxi 
         bmtrx(i,1,1,19)=dn4dxi 
c 
         bmtrx(i,1,1,5) =coef*dn1dxi 
         bmtrx(i,1,1,11)=coef*dn2dxi 
         bmtrx(i,1,1,17)=coef*dn3dxi 
         bmtrx(i,1,1,23)=coef*dn4dxi 
c 
         bmtrx(i,1,2,1) =dn1deta 
         bmtrx(i,1,2,7) =dn2deta 
         bmtrx(i,1,2,13)=dn3deta 
         bmtrx(i,1,2,19)=dn4deta 
c 
         bmtrx(i,1,2,5) =coef*dn1deta 
         bmtrx(i,1,2,11)=coef*dn2deta 
         bmtrx(i,1,2,17)=coef*dn3deta 
         bmtrx(i,1,2,23)=coef*dn4deta 
c 
         bmtrx(i,2,1,2) =dn1dxi 
         bmtrx(i,2,1,8) =dn2dxi 
         bmtrx(i,2,1,14)=dn3dxi 
         bmtrx(i,2,1,20)=dn4dxi 
c 
         bmtrx(i,2,1,4) =-coef*dn1dxi 
         bmtrx(i,2,1,10)=-coef*dn2dxi 
         bmtrx(i,2,1,16)=-coef*dn3dxi 
         bmtrx(i,2,1,22)=-coef*dn4dxi
APPENDIX C 
c 
         bmtrx(i,1,3,5) =.5*thick(i)*n1 
         bmtrx(i,1,3,11)=.5*thick(i)*n2 
         bmtrx(i,1,3,17)=.5*thick(i)*n3 
         bmtrx(i,1,3,23)=.5*thick(i)*n4 
c 
         bmtrx(i,3,1,3) =dn1dxi 
         bmtrx(i,3,1,9) =dn2dxi 
         bmtrx(i,3,1,15)=dn3dxi 
         bmtrx(i,3,1,21)=dn4dxi 
c 
         bmtrx(i,2,2,2) =dn1deta 
         bmtrx(i,2,2,8) =dn2deta 
         bmtrx(i,2,2,14)=dn3deta 
         bmtrx(i,2,2,20)=dn4deta 
c 
         bmtrx(i,2,2,4) =-coef*dn1deta 
         bmtrx(i,2,2,10)=-coef*dn2deta 
         bmtrx(i,2,2,16)=-coef*dn3deta 
         bmtrx(i,2,2,22)=-coef*dn4deta 
c 
         bmtrx(i,2,3,4) =-.5*thick(i)*n1 
         bmtrx(i,2,3,10)=-.5*thick(i)*n2 
         bmtrx(i,2,3,16)=-.5*thick(i)*n3 
         bmtrx(i,2,3,22)=-.5*thick(i)*n4 
c 
         bmtrx(i,3,2,3) =dn1deta 
         bmtrx(i,3,2,9) =dn2deta 
         bmtrx(i,3,2,15)=dn3deta 
         bmtrx(i,3,2,21)=dn4deta 
c 
      enddo 
c 
      return 
      end 
To use the element for a part the section card can be written as 
*SECTION_SHELL 
$    SECID    ELFORM 
         1       101 
$       T1        T2        T3        T4 
$     NIPP     NXDOF      IUNF      IHGF 
         1         0         0         1 
$       XI       ETA       WGT 
        0.        0.        4. 
Sample User Solid Element 101 (constant stress solid) 
The geometry for the constant stress solid is given as 
𝑥𝑖 = 𝑥𝑖𝐼𝑁𝐼(𝜉1, 𝜉2) 
𝑣𝑖 = 𝑣𝑖𝐼𝑁𝐼(𝜉1, 𝜉2) 
where, 
𝑥𝑖𝐼 = 𝑖th component of coordinate of node 𝐼 
𝑣𝑖𝐼 = 𝑖th component of translational velocity of node 𝐼 
𝑁𝐼 = shape function localized at node 𝐼
APPENDIX C 
The  matrices  necessary  for  implementing  this  element  as  a  user-defined  solid  are 
derived from the expressions given by 
and, 
∂𝑥𝑖
∂𝜉1
∂𝑥𝑖
∂𝜉2
∂𝑥𝑖
∂𝜉3
∂𝑣𝑖
∂𝜉1
∂𝑣𝑖
∂𝜉2
∂𝑣𝑖
∂𝜉3
= 𝑥𝑖𝐼
= 𝑥𝑖𝐼
= 𝑥𝑖𝐼
= 𝑣𝑖𝐼
= 𝑣𝑖𝐼
= 𝑣𝑖𝐼
∂𝑁𝐼
∂𝜉1
∂𝑁𝐼
∂𝜉2
∂𝑁𝐼
∂𝜉3
∂𝑁𝐼
∂𝜉1
∂𝑁𝐼
∂𝜉2
∂𝑁𝐼
∂𝜉3
The user element implementation is given by 
      subroutine usld_b101(bmtrx,gmtrx,gjac, 
     1     xi,eta,zeta, 
     2     n1,n2,n3,n4,n5,n6,n7,n8, 
     3     dn1dxi,dn2dxi,dn3dxi,dn4dxi, 
     4     dn5dxi,dn6dxi,dn7dxi,dn8dxi, 
     5     dn1deta,dn2deta,dn3deta,dn4deta, 
     6     dn5deta,dn6deta,dn7deta,dn8deta, 
     7     dn1dzeta,dn2dzeta,dn3dzeta,dn4dzeta, 
     8     dn5dzeta,dn6dzeta,dn7dzeta,dn8dzeta, 
     9     x1,x2,x3,x4,x5,x6,x7,x8, 
     .     y1,y2,y3,y4,y5,y6,y7,y8, 
     .     z1,z2,z3,z4,z5,z6,z7,z8, 
     .     xdof, 
     .     lft,llt) 
      include 'nlqparm' 
c 
c     Compute b and g matrix for user-defined solid 101 
c 
      dimension bmtrx(nlq,3,3,*),gmtrx(nlq,3,3),gjac(nlq) 
      REAL n1,n2,n3,n4,n5,n6,n7,n8 
      dimension x1(nlq),x2(nlq),x3(nlq),x4(nlq) 
      dimension x5(nlq),x6(nlq),x7(nlq),x8(nlq) 
      dimension y1(nlq),y2(nlq),y3(nlq),y4(nlq) 
      dimension y5(nlq),y6(nlq),y7(nlq),y8(nlq) 
      dimension z1(nlq),z2(nlq),z3(nlq),z4(nlq) 
      dimension z5(nlq),z6(nlq),z7(nlq),z8(nlq) 
      dimension xdof(nlq,8,3) 
c 
      do i=lft,llt 
c 
         gmtrx(i,1,1)=x1(i)*dn1dxi+x2(i)*dn2dxi+ 
     1        x3(i)*dn3dxi+x4(i)*dn4dxi+
APPENDIX C 
     2        x5(i)*dn5dxi+x6(i)*dn6dxi+ 
     3        x7(i)*dn7dxi+x8(i)*dn8dxi 
         gmtrx(i,2,1)=y1(i)*dn1dxi+y2(i)*dn2dxi+ 
     1        y3(i)*dn3dxi+y4(i)*dn4dxi+ 
     2        y5(i)*dn5dxi+y6(i)*dn6dxi+ 
     3        y7(i)*dn7dxi+y8(i)*dn8dxi 
         gmtrx(i,3,1)=z1(i)*dn1dxi+z2(i)*dn2dxi+ 
     1        z3(i)*dn3dxi+z4(i)*dn4dxi+ 
     2        z5(i)*dn5dxi+z6(i)*dn6dxi+ 
     3        z7(i)*dn7dxi+z8(i)*dn8dxi 
         gmtrx(i,1,2)=x1(i)*dn1deta+x2(i)*dn2deta+ 
     1        x3(i)*dn3deta+x4(i)*dn4deta+ 
     2        x5(i)*dn5deta+x6(i)*dn6deta+ 
     3        x7(i)*dn7deta+x8(i)*dn8deta 
         gmtrx(i,2,2)=y1(i)*dn1deta+y2(i)*dn2deta+ 
     1        y3(i)*dn3deta+y4(i)*dn4deta+ 
     2        y5(i)*dn5deta+y6(i)*dn6deta+ 
     3        y7(i)*dn7deta+y8(i)*dn8deta 
         gmtrx(i,3,2)=z1(i)*dn1deta+z2(i)*dn2deta+ 
     1        z3(i)*dn3deta+z4(i)*dn4deta+ 
     2        z5(i)*dn5deta+z6(i)*dn6deta+ 
     3        z7(i)*dn7deta+z8(i)*dn8deta 
         gmtrx(i,1,3)=x1(i)*dn1dzeta+x2(i)*dn2dzeta+ 
     1        x3(i)*dn3dzeta+x4(i)*dn4dzeta+ 
     2        x5(i)*dn5dzeta+x6(i)*dn6dzeta+ 
     3        x7(i)*dn7dzeta+x8(i)*dn8dzeta 
         gmtrx(i,2,3)=y1(i)*dn1dzeta+y2(i)*dn2dzeta+ 
     1        y3(i)*dn3dzeta+y4(i)*dn4dzeta+ 
     2        y5(i)*dn5dzeta+y6(i)*dn6dzeta+ 
     3        y7(i)*dn7dzeta+y8(i)*dn8dzeta 
         gmtrx(i,3,3)=z1(i)*dn1dzeta+z2(i)*dn2dzeta+ 
     1        z3(i)*dn3dzeta+z4(i)*dn4dzeta+ 
     2        z5(i)*dn5dzeta+z6(i)*dn6dzeta+ 
     3        z7(i)*dn7dzeta+z8(i)*dn8dzeta 
c 
         bmtrx(i,1,1,1) =dn1dxi 
         bmtrx(i,1,1,4) =dn2dxi 
         bmtrx(i,1,1,7) =dn3dxi 
         bmtrx(i,1,1,10)=dn4dxi 
         bmtrx(i,1,1,13)=dn5dxi 
         bmtrx(i,1,1,16)=dn6dxi 
         bmtrx(i,1,1,19)=dn7dxi 
         bmtrx(i,1,1,22)=dn8dxi 
c 
         bmtrx(i,2,1,2) =dn1dxi 
         bmtrx(i,2,1,5) =dn2dxi 
         bmtrx(i,2,1,8) =dn3dxi 
         bmtrx(i,2,1,11)=dn4dxi 
         bmtrx(i,2,1,14)=dn5dxi 
         bmtrx(i,2,1,17)=dn6dxi 
         bmtrx(i,2,1,20)=dn7dxi 
         bmtrx(i,2,1,23)=dn8dxi 
c 
         bmtrx(i,3,1,3) =dn1dxi 
         bmtrx(i,3,1,6) =dn2dxi 
         bmtrx(i,3,1,9) =dn3dxi 
         bmtrx(i,3,1,12)=dn4dxi 
         bmtrx(i,3,1,15)=dn5dxi 
         bmtrx(i,3,1,18)=dn6dxi 
         bmtrx(i,3,1,21)=dn7dxi 
         bmtrx(i,3,1,24)=dn8dxi 
c 
         bmtrx(i,1,2,1) =dn1deta 
         bmtrx(i,1,2,4) =dn2deta 
         bmtrx(i,1,2,7) =dn3deta 
         bmtrx(i,1,2,10)=dn4deta
APPENDIX C 
         bmtrx(i,1,2,13)=dn5deta 
         bmtrx(i,1,2,16)=dn6deta 
         bmtrx(i,1,2,19)=dn7deta 
         bmtrx(i,1,2,22)=dn8deta 
c 
         bmtrx(i,2,2,2) =dn1deta 
         bmtrx(i,2,2,5) =dn2deta 
         bmtrx(i,2,2,8) =dn3deta 
         bmtrx(i,2,2,11)=dn4deta 
         bmtrx(i,2,2,14)=dn5deta 
         bmtrx(i,2,2,17)=dn6deta 
         bmtrx(i,2,2,20)=dn7deta 
         bmtrx(i,2,2,23)=dn8deta 
c 
         bmtrx(i,3,2,3) =dn1deta 
         bmtrx(i,3,2,6) =dn2deta 
         bmtrx(i,3,2,9) =dn3deta 
         bmtrx(i,3,2,12)=dn4deta 
         bmtrx(i,3,2,15)=dn5deta 
         bmtrx(i,3,2,18)=dn6deta 
         bmtrx(i,3,2,21)=dn7deta 
         bmtrx(i,3,2,24)=dn8deta 
c 
         bmtrx(i,1,3,1) =dn1dzeta 
         bmtrx(i,1,3,4) =dn2dzeta 
         bmtrx(i,1,3,7) =dn3dzeta 
         bmtrx(i,1,3,10)=dn4dzeta 
         bmtrx(i,1,3,13)=dn5dzeta 
         bmtrx(i,1,3,16)=dn6dzeta 
         bmtrx(i,1,3,19)=dn7dzeta 
         bmtrx(i,1,3,22)=dn8dzeta 
c 
         bmtrx(i,2,3,2) =dn1dzeta 
         bmtrx(i,2,3,5) =dn2dzeta 
         bmtrx(i,2,3,8) =dn3dzeta 
         bmtrx(i,2,3,11)=dn4dzeta 
         bmtrx(i,2,3,14)=dn5dzeta 
         bmtrx(i,2,3,17)=dn6dzeta 
         bmtrx(i,2,3,20)=dn7dzeta 
         bmtrx(i,2,3,23)=dn8dzeta 
c 
         bmtrx(i,3,3,3) =dn1dzeta 
         bmtrx(i,3,3,6) =dn2dzeta 
         bmtrx(i,3,3,9) =dn3dzeta 
         bmtrx(i,3,3,12)=dn4dzeta 
         bmtrx(i,3,3,15)=dn5dzeta 
         bmtrx(i,3,3,18)=dn6dzeta 
         bmtrx(i,3,3,21)=dn7dzeta 
         bmtrx(i,3,3,24)=dn8dzeta 
c 
      enddo 
c 
      return 
      end 
To use the element for a part the section card can be written as 
*SECTION_SOLID 
$    SECID    ELFORM 
         1       101 
$      NIP     NXDOF      IHGF  
         1         0         1  
$       XI       ETA      ZETA       WGT 
        0.        0.        0.       8.0
APPENDIX C 
Examples 
We present three test examples. 
One example was a simple tension-compression test of a solid cylinder.  The geometry 
is  shown  in  Figure  46-1.    The  problem  is  using  the  sample  implementations  of  user 
elements and compared the results and performance with standard LS-DYNA elements.  
As  for  the  computational  efficiency,  we  note  that  the  performance  is  worse  but  this  is 
expected  since  there  is  little  room  for  optimization  of  the  code  while  retaining  a  user 
friendly interface.  The implicit performance compares well with the other elements in 
LS-DYNA. 
The  second  example  was  a  combined  bending  and  stretching  example  with  the 
geometry  shown  in  Figure  46-2.    Again  we  ran  the  problem  with  the  user  element 
implementations  and  compared  the  results  and  performance  with  standard  LS-DYNA 
elements.  We could see the same tendencies as for the solid elements. 
The third and final example is an impact between a solid bar and shell beam.  Both parts 
are  modeled  with  user-defined  elements.    The  results  were  very  similar  to  the  ones 
obtained  by  substituting  the  sections  for  standard  LS-DYNA  sections,  but  the 
simulation time was about 3-4 times longer.
APPENDIX C 
Figure 46-1.  Solid mesh for user element test. 
Figure 46-2.  Shell mesh for the user element test.
APPENDIX C 
Figure 46-3.  Impact between a user-defined shell and user-defined solid part.
APPENDIX D 
APPENDIX D:  User Defined 
Airbag Sensor 
The addition of a user sensor subroutine into LS-DYNA is relatively simple.  The sensor 
is mounted on a rigid body which is attached to the structure.  The motion of the sensor 
is provided in the local coordinate system defined for the rigid body in the definition of 
material  model  20–the  rigid  material.    When  the  user  defined  criterion  is  met  for  the 
deployment  of  the  airbag,  a  flag  is  set  and  the  deployment  begins.    All  load  curves 
relating  to  the  mass  flow  rate  versus  time  are  then  shifted  by  the  initiation  time.    The 
user  subroutine  is  given  below  with  all  the  necessary  information  contained  in  the 
comment cards. 
      subroutine airusr (rbu,rbv,rba,time,dt1,dt2,param,hist,itrnon, 
     .  rbug,rbvg,rbag,icnv) 
c 
c****************************************************************** 
c|  Livermore Software Technology Corporation  (LSTC)             | 
c|  ------------------------------------------------------------  | 
c|  Copyright 1987-2008 Livermore Software Tech.  Corp             | 
c|  All rights reserved                                           | 
c****************************************************************** 
c 
c     user subroutine to initiate the inflation of the airbag 
c 
c     variables 
c 
c     displacements are defined at time n+1 in local system 
c     velocites are defined at time n+1/2 in local system 
c     accelerations are defined at time n in local system 
c 
c         rbu(1-3) total displacements in the local xyz directions 
c         rbu(3-6) total rotations about the local xyz axes 
c         rbv(1-3) velocities in the local xyz directions 
c         rbv(3-6) rotational velocities about the local xyz axes 
c         rba(1-3) accelerations in the local xyz directions 
c         rba(3-6) rotational accelerations about the local xyz axes 
c         time is the current time 
c         dt1 is time step size at n-1/2 
c         dt2 is time step size at n+1/2 
c         param is user defined input parameters 
c         hist is user defined history variables 
c         itrnon is a flag to turn on the airbag inflation 
c         rbug,rbvg,rbag, are similar to rbu,rbv,rba but are defined 
c                         globally. 
c         icnv is the airbag ID 
c 
c     the user subroutine sets the variable itrnon to: 
c 
c           itrnon=0 bag is not inflated 
c           itrnon=1 bag inflation begins and this subroutine is 
c                    not called again 
c 
      include 'iounits.inc' 
      dimension rbu(6),rbv(6),rba(6),param(25),hist(25), 
     .  rbug(6),rbvg(6),rbag(6) 
c 
      itrnon=0 
      ra=sqrt(rba(1)**2+rba(2)**2+rba(3)**2) 
      if (ra.gt.param(1)) then
APPENDIX D 
        itrnon=1 
        write(iotty,100) time 
        write(iohsp,100) time 
        write(iomsg,100) time 
      endif 
 100  format (' Airbag activated at time ',1pe10.3) 
c 
      return 
      end
APPENDIX E 
APPENDIX E:  User Defined 
Solution Control 
This  subroutine may  be provided by the user to control the I/O, monitor the energies 
and  other  solution  norms  of  interest,  and  to  shut  down  the  problem  whenever  he 
pleases.    The  arguments  are  defined  in  the  listing  provided  below.    This  subroutine  is 
called each time step and does not need any control card to operate. 
      subroutine uctrl1 (numnp,ndof,time,dt1,dt2,prtc,pltc,frci,prto, 
     .  plto,frco,vt,vr,at,ar,ut,ur,xmst,xmsr,irbody,rbdyn,usrhv, 
     .  messag,totalm,cycle,idrint,mtype,mxrb,nrba,rbcor,x,rbv,nrbn, 
     .  nrb,xrb,yrb,zrb,axrb,ayrb,azrb,dtx,nmmat,rba,fvalnew,fvalold, 
     .  fvalmid,fvalnxt) 
c 
c****************************************************************** 
c|  Livermore Software Technology Corporation  (LSTC)             | 
c|  ------------------------------------------------------------  | 
c|  Copyright 1987-2008 Livermore Software Tech.  Corp             | 
c|  All rights reserved                                           | 
c****************************************************************** 
c 
c     user subroutine for solution control and is called at the 
c     beginning of time step n+1.   The time at n+ 
c 
c 
c     note:  ls-dyna3d uses an internal numbering system to 
c            accomodate arbitrary node numbering.   to access 
c            information for user node n, address array location m, 
c            m = lqf8(n,1).  to obtain user node number, n, 
c            corresponding to array address m, set n = lqfinv(m,1) 
c 
c     arguments: 
c          numnp = number of nodal points 
c          ndof = number of degrees of freedom per node 
c          time = current solution time at n+1 
c          dt1  = time step size between time n-1 and n 
c          dt2  = time step size between time n and n+1 
c          prtc = output interval for taurus time history data 
c          pltc = output interval for taurus state data 
c          frci = output interval for taurus interface force data 
c          prto = output time for time history file 
c          plto = output time for state data 
c          frco = output time for force data 
c          vt(3,numnp) = nodal translational velocity vector 
c          vr(3,numnp) = nodal rotational velocity vector.  this 
c                       array is defined if and only if ndof = 6 
c          at(3,numnp) = nodal translational acceleration vector 
c          ar(3,numnp) = nodal rotational acceleration vector.  this 
c                       array is defined if and only if ndof = 6 
c          ut(3,numnp) = nodal translational displacement vector 
c          ur(3,numnp) = nodal rotational displacement vector.  this 
c                       array is defined if and only if ndof = 6 
c          xmst(numnp) = reciprocal of nodal translational masses 
c          xmsr(numnp) = reciprocal of nodal rotational masses.  this 
c                       array is defined if and only if ndof = 6
APPENDIX E 
c          fvalold     = array for storing load curve values at time n 
c          fvalnew     = array for setting load curve values at time n+1 
c                       only load curves with 0 input points may be user 
c                       defined.  When the load curve is user set, the 
c                       value at time n must be stored in array fvalold. 
c          fvalmid     = array for predicting load curve values at time n+3/2 
c          fvalnxt     = array for predicting load curve values at time n+2 
c                       for some applications it is necessary to predict the 
c                       load curve values at time n+2, a time that is not 
known, 
c                       this for instance for boundary prescribed motion.  In 
c                       this case the load curve values at time n+3/2 need to 
c                       be predicted in fvalmid, and fvalold should be set to 
c                       fvalnew and fvalnew should be set to fvalnxt.  See 
c                       coding below. 
c 
c          irbody      = 0 if no rigid bodies 
c          rbdyn(numnp)=flag for rigid body nodal points 
c                       if deformable node then set to 1.0 
c                       if rigid body node then set to 0.0 
c                       defined if and only if rigid bodies are present 
c                       i.e., irbody.ne.0 if no rigid bodies are 
c                       present 
c          usrhv(lenhv)=user defined history variables that are stored 
c                       in the restart file.  lenhv = 100+7*nummat where 
c                       nummat is the # of materials in the problem. 
c                       array usrhv is updated only in this subroutine. 
c          messag      = flag for dyna3d which may be set to: 
c                      'sw1.' ls-dyna3d terminates with restart file 
c                      'sw3.' ls-dyna3d writes a restart file 
c                     'sw4.' ls-dyna3d writes a plot state 
c           totalm     = total mass in problem 
c           cycle      = cycle number 
c           idrint     = flag for dynamic relaxation phase 
c                       .ne.0: dynamic relaxation in progress 
c                       .eq.0: solution phase 
c 
      include 'ptimes.inc' 
c 
c     prtims(1-37)=output intervals for ascii files 
c 
c      ascii files: 
c           ( 1)-cross section forces 
c           ( 2)-rigid wall forces 
c           ( 3)-nodal data 
c           ( 4)-element data 
c           ( 5)-global data 
c           ( 6)-discrete elements 
c           ( 7)-material energies 
c           ( 8)-noda interface forces 
c           ( 9)-resultant interface forces 
c           (10)-smug animator 
c           (11)-spc reaction forces 
c           (12)-nodal constraint resultant forces 
c           (13)-airbag statistics 
c           (14)-avs database 
c           (15)-nodal force groups 
c           (16)-output intervals for nodal boundary conditions 
c           (17)-(32) unused at this time 
c           (37)-auto tiebreak damage output
APPENDIX E 
c 
c     prtlst(32)=output times for ascii files above.  when solution time 
c                exceeds the output time a print state is dumped. 
c 
      common/rbkeng/enrbdy,rbdyx,rbdyy,rbdyz 
c 
c      total rigid body energies and momentums: 
c           enrbdy = rigid body kinetic energy 
c           rbdyx = rigid body x-momentum 
c           rbdyy = rigid body y-momentum 
c           rbdyz = rigid body z-momentum 
c 
      common/swmke/swxmom,swymom,swzmom,swkeng 
c 
c      total stonewall energies and momentums: 
c           swxmom = stonewall x-momentum 
c           swymom = stonewall y-momentum 
c           swzmom = stonewall z-momentum 
c           swkeng = stonewall kinetic energy 
c 
      common/deengs/deeng 
c 
c      deeng = total discrete element energy 
c 
      common/bk28/summss,xke,xpe,tt,xte0,erodeke,erodeie,selie,selke, 
     .  erodehg 
c 
c      xpe  = total internal energy in the finite elements 
c 
      common/sprengs/spreng 
c 
c      spreng = total spr energy 
c 
      character*(*) messag 
      integer cycle 
      real*8 x 
      dimension vt(3,*),vr(3,*),at(3,*),ar(3,*), 
     .  xmst(*),xmsr(*),rbdyn(*),usrhv(*),mtype(*),mxrb(*),nrba(*), 
     .  rbcor(3,1),x(*),rbv(6,*),nrbn(*),nrb(*),xrb(*),yrb(*), 
     .  zrb(*),axrb(*),ayrb(*),azrb(*),rba(6,*),fvalnew(*), 
     .  fvalold(*),fvalmid(*),fvalnxt(*) 
      real*8 ut(3,*),ur(3,*) 
c 
c     sample momentum and kinetic energy calculations 
c 
c     remove all comments in column 1 below to activate 
      i = 1 
      if (i.eq.1) return 
c     return 
cc 
cc 
cc     initialize kinetic energy, xke, and x,y,z momentums. 
cc 
c      xke = 2.*swkeng+2.*enrbdy 
c      xm = swxmom+rbdyx 
c      ym = swymom+rbdyy 
c      zm = swzmom+rbdyz 
cc 
c      numnp2 = numnp 
c      if (ndof.eq.6) then
APPENDIX E 
c        numnp2 = numnp+numnp 
c      endif 
c      write(iotty,*)ndof 
cc 
cc 
cc     no rigid bodies present 
cc 
c      if (irbody.eq.0) then 
cc       note in blank comment vr follows vt.  this fact is used below. 
c        do 10 n = 1,numnp2 
c        xmsn = 1./xmst(n) 
c        vn1 = vt(1,n) 
c        vn2 = vt(2,n) 
c        vn3 = vt(3,n) 
c        xm = xm+xmsn*vn1 
c        ym = ym+xmsn*vn2 
c        zm = zm+xmsn*vn3 
c        xke = xke+xmsn*(vn1*vn1+vn2*vn2+vn3*vn3) 
c   10   continue 
cc 
cc 
cc     rigid bodies present 
cc 
c      else 
cc       nodal accerations for rigid bodies 
cc 
c        do 12 n = 1,nmmat 
c        if (mtype(n).ne.20.or.mxrb(n).ne.n) go to 12 
c        lrbn = nrba(n) 
c        call stvlut(rbcor(1,n),x,vt,at,ar,vr,rbv(1,n),dt2, 
c    .   nrbn(n),nrb(lrbn),xrb,yrb,zrb,axrb,ayrb,azrb,dtx) 
c 
c        rigid body nodal accelerations 
c 
c        if (ndof.eq.6) then 
c          call rbnacc(nrbn(n),nrb(lrbn),rba(4,n),ar) 
c        endif 
c 
c  12    continue 
cc 
c        do 20 n = 1,numnp 
c        xmsn = 1./xmst(n) 
c        vn1 = rbdyn(n)*vt(1,n) 
c        vn2 = rbdyn(n)*vt(2,n) 
c        vn3 = rbdyn(n)*vt(3,n) 
c        xm = xm+xmsn*vn1 
c        ym = ym+xmsn*vn2 
c        zm = zm+xmsn*vn3 
c        xke = xke+xmsn*(vn1*vn1+vn2*vn2+vn3*vn3) 
c   20   continue 
c        if (ndof.eq.6) then 
c          do 30 n = 1,numnp 
c          xmsn = 1./xmsr(n) 
c          vn1 = rbdyn(n)*vr(1,n) 
c          vn2 = rbdyn(n)*vr(2,n) 
c          vn3 = rbdyn(n)*vr(3,n) 
c          xm = xm+xmsn*vn1 
c          ym = ym+xmsn*vn2 
c          zm = zm+xmsn*vn3 
c          xke = xke+xmsn*(vn1*vn1+vn2*vn2+vn3*vn3)
APPENDIX E 
c   30     continue 
c        endif 
c      endif 
cc 
cc     total kinetic energy 
c      xke=.5*xke 
cc     total internal energy 
c      xie = xpe+deeng+spreng 
cc     total energy 
c      xte = xke+xpe+deeng+spreng 
cc     total x-rigid body velocity 
c      xrbv = xm/totalm 
cc     total y-rigid body velocity 
c      yrbv = ym/totalm 
cc     total z-rigid body velocity 
c      zrbv = zm/totalm 
       return 
       end
APPENDIX F 
APPENDIX F:  User Defined 
Interface Control 
This  subroutine  may  be  provided  by  the  user  to  turn  the  interfaces  on  and  off.    This 
option  is  activated  by  the  *USER_INTERFACE_CONTROL  keyword.    The  arguments 
are defined in the listing provided below. 
      subroutine uctrl2(nsi,nty,time,cycle,msr,nmn,nsv,nsn, 
     1 thmr,thsv,vt,xi,ut,iskip,idrint,numnp,dt2,ninput,ua, 
     2 irectm,nrtm,irects,nrts) 
c 
c****************************************************************** 
c|  Livermore Software Technology Corporation  (LSTC)             | 
c|  ------------------------------------------------------------  | 
c|  Copyright 1987-2008 Livermore Software Tech.  Corp             | 
c|  All rights reserved                                           | 
c****************************************************************** 
c 
c     user subroutine for interface control 
c 
c     note:  ls-dyna3d uses an internal numbering system to 
c            accomodate arbitrary node numbering.   to access 
c            information for user node n, address array location m, 
c            m = lqf8(n,1).  to obtain user node number, n, 
c            corresponding to array address m, set n = lqfinv(m,1) 
c 
c     arguments: 
c          nsi        = number of sliding interface 
c          nty        = interface type. 
c                      .eq.4:single surface 
c                      .ne.4:surface to surface 
c          time       = current solution time 
c          cycle      = cycle number 
c          msr(nmn)   = list of master nodes numbers in internal 
c                      numbering scheme 
c          nmn        = number of master nodes 
c          nsv(nsn)   = list of slave nodes numbers in internal 
c                      numbering scheme 
c          nsn        = number of slave nodes 
c          thmr(nmn)  = master node thickness 
c          thsv(nsn)  = slave node thickness 
c          vt(3,numnp)=nodal translational velocity vector 
c          xi(3,numnp)=initial coordinates at time = 0 
c          ut(3,numnp)=nodal translational displacement vector 
c          idrint     = flag for dynamic relaxation phase 
c                      .ne.0: dynamic relaxation in progress 
c                      .eq.0: solution phase 
c          numnp      = number of nodal points 
c          dt2        = time step size at n+1/2 
c          ninput     = number of variables input into ua 
c          ua(*)      = users' array, first ninput locations 
c                      defined by user.  the length of this 
c                      array is defined on control card 10. 
c                      this array is unique to interface nsi. 
c          irectm(4,*)=list of master segments in internal
APPENDIX F 
c                      numbering scheme 
c          nrtm       = number of master segments 
c          irects(4,*)=list of slave segments in internal 
c                      numbering scheme 
c          nrts       = number of master segments 
c 
c     set flag for active contact 
c       iskip = 0 active 
c       iskip = 1 inactive 
c 
c******************************************************************* 
c 
      integer cycle 
      real*8 ut 
      real*8 xi 
      dimension msr(*),nsv(*),thmr(*),thsv(*),vt(3,*),xi(3,*), 
     .          ut(3,*),ua(*),irectm(4,*),irects(4,*) 
c 
c     the following sample of codeing is provided to illustrate how 
c     this subroutine might be used.   here we check to see if the 
c     surfaces in the surface to surface contact are separated.   if 
c     so the iskip = 1 and the contact treatment is skipped. 
c 
c     if (nty.eq.4) return 
c     dt2hlf = dt2/2. 
c     xmins = 1.e+16 
c     xmaxs = -xmins 
c     ymins = 1.e+16 
c     ymaxs = -ymins 
c     zmins = 1.e+16 
c     zmaxs = -zmins 
c     xminm = 1.e+16 
c     xmaxm = -xminm 
c     yminm = 1.e+16 
c     ymaxm = -yminm 
c     zminm = 1.e+16 
c     zmaxm = -zminm 
c     thks = 0.0 
c     thkm = 0.0 
c     do 10 i = 1,nsn 
c     dsp1 = ut(1,nsv(i))+dt2hlf*vt(1,nsv(i)) 
c     dsp2 = ut(2,nsv(i))+dt2hlf*vt(2,nsv(i)) 
c     dsp3 = ut(3,nsv(i))+dt2hlf*vt(3,nsv(i)) 
c     x1 = xi(1,nsv(i))+dsp1 
c     x2 = xi(2,nsv(i))+dsp2 
c     x3 = xi(3,nsv(i))+dsp3 
c     thks = max(thsv(i),thks) 
c     xmins = min(xmins,x1) 
c     xmaxs = max(xmaxs,x1) 
c     ymins = min(ymins,x2) 
c     ymaxs = max(ymaxs,x2) 
c     zmins = min(zmins,x3) 
c     zmaxs = max(zmaxs,x3) 
c  10 continue 
c     do 20 i = 1,nmn 
c     dsp1 = ut(1,msr(i))+dt2hlf*vt(1,msr(i)) 
c     dsp2 = ut(2,msr(i))+dt2hlf*vt(2,msr(i)) 
c     dsp3 = ut(3,msr(i))+dt2hlf*vt(3,msr(i)) 
c     x1 = xi(1,msr(i))+dsp1 
c     x2 = xi(2,msr(i))+dsp2
APPENDIX F 
c     x3 = xi(3,msr(i))+dsp3 
c     thkm = max(thmr(i),thks) 
c     xminm = min(xminm,x1) 
c     xmaxm = max(xmaxm,x1) 
c     yminm = min(yminm,x2) 
c     ymaxm = max(ymaxm,x2) 
c     zminm = min(zminm,x3) 
c     zmaxm = max(zmaxm,x3) 
c  20 continue 
c 
c     if thks or thkm equal zero set them to some reasonable value 
c 
c     if (thks.eq.0.0) then 
c       e1=(xi(1,irects(1,1))-xi(1,irects(3,1)))**2 
c    .    +(xi(2,irects(1,1))-xi(2,irects(3,1)))**2 
c    .    +(xi(3,irects(1,1))-xi(3,irects(3,1)))**2 
c       e2=(xi(1,irects(2,1))-xi(1,irects(4,1)))**2 
c    .    +(xi(2,irects(2,1))-xi(2,irects(4,1)))**2 
c    .    +(xi(3,irects(2,1))-xi(3,irects(4,1)))**2 
c       thks=.3*sqrt(max(e1,e2)) 
c     endif 
c     if (thkm.eq.0.0) then 
c       e1=(xi(1,irectm(1,1))-xi(1,irectm(3,1)))**2 
c    .    +(xi(2,irectm(1,1))-xi(2,irectm(3,1)))**2 
c    .    +(xi(3,irectm(1,1))-xi(3,irectm(3,1)))**2 
c       e2=(xi(1,irectm(2,1))-xi(1,irectm(4,1)))**2 
c    .    +(xi(2,irectm(2,1))-xi(2,irectm(4,1)))**2 
c    .    +(xi(3,irectm(2,1))-xi(3,irectm(4,1)))**2 
c       thkm=.3*sqrt(max(e1,e2)) 
c     endif 
c 
c     if (xmaxs+thks.lt.xminm-thkm) go to 40 
c     if (ymaxs+thks.lt.yminm-thkm) go to 40 
c     if (zmaxs+thks.lt.zminm-thkm) go to 40 
c     if (xmaxm+thkm.lt.xmins-thks) go to 40 
c     if (ymaxm+thkm.lt.ymins-thks) go to 40 
c     if (zmaxm+thkm.lt.zmins-thks) go to 40 
c     iskip = 0 
c 
c     return 
c  40 iskip = 1 
c 
      return 
      end
APPENDIX G 
APPENDIX G:  User Defined Interface 
Friction and Conductivity 
An  easy-to-use  user  contact  interface  is  provided  in  LS-DYNA  where  the  user  has  the 
possibility  to  define  the  frictional  coefficients  (static  and  dynamic)  as  well  as  contact 
heat  transfer  conductance  as  functions  of  contact  pressure,  relative  sliding  velocity, 
separation and temperature.  To be able to use this feature, an object version of the LS-
DYNA  code  is  required  and  the  user  must  write  his/her  own  Fortran  (or  C)  code  to 
define the contact parameters of interest.  
In the text file dyn21.f that comes with the object version of LS-DYNA, the subroutines 
of interest are 
subroutine usrfrc(fstt,fdyn,...) 
for defining the frictional coefficients fstt (static) and fdyn (dynamic) and 
subroutine usrhcon(h,...) 
for defining the heat transfer contact conductance h.  
We  emphasize  at  this  point  that  the  user  friction  interface  differs  between  LS-DYNA 
(SMP)  and  MPP-DYNA  (MPP),  for  reasons  that  have  to  do  with  how  the  contacts  are 
implemented in general.  In LS-DYNA (SMP) the user is required not only to define the 
frictional coefficients but also to assemble and store contact forces and history, whereas 
in MPP-DYNA (MPP) only the frictional coefficients have to be defined.  
For the friction interface (SMP and MPP) the user may associate history variables with 
each contact node.  Unfortunately, the user friction interface is currently not supported 
by  all  available  contacts  in  LS-DYNA  and  MPP-DYNA,  but  it  should  cover  the  most 
interesting  ones  among  others,  *CONTACT_(FORMING_)NODES_TO_SURFACE, 
*CONTACT_(FORMING_)SURFACE_TO_SURFACE,  *CONTACT_(FORMING_)ONE_
WAY_SURFACE_TO_SURFACE.  Upon request by customers additional contact types 
can be supported.  
One of the arguments to the user contact routines is the curve array crv, also available 
in the user material interface.  Note that when using this array, the curve identity must 
be  converted  to  an  internal  number  or  the  subroutine  crvval  may  be  utilized.    For 
more information, see the appendix A on user materials. 
For definition of user contact parameters the user must define the keywords 
*USER_INTERFACE_FRICTION 
or 
*USER_INTERFACE_CONDUCTIVITY
APPENDIX G 
The card format for these two keywords are identical and can be found in other sections 
in this manual.  
There  is  an  alternate  route  to  defining  the  conductivity  parameters  for  a  user  defined 
thermal  contact.    On  the  *CONTACT_..._THERMAL_FRICTION  optional  card  the 
parameter FORMULA may be set to a negative number.  This will automatically create 
a  user  defined  conductivity  interface  and  invoke  reading  of  –FORMULA  contact 
parameters immediately following the card including the FORMULA parameter.  Note 
that  FORMULA  is  related  to  NOC  and  NOCI  in  the  *USER_INTERFACE_CONDUC-
TIVITY keyword as  
– FORMULA = NOC = NOCI. 
Note that the pressure is automatically computed for each  user conductivity interface, 
i.e., the keyword *LOAD_SURFACE_STRESS is not necessary. 
A sample friction subroutine is provided below for SMP. 
      subroutine usrfrc(nosl,time,ncycle,dt2,insv,areas,xs,ys,zs, 
     .  lsv,ix1,ix2,ix3,ix4,aream,xx1,xx2,xx3,stfn,stf,fni, 
     .  dx,dy,dz,fdt2,ninput,ua,side,iisv5,niisv5,n1,n2,n3,fric1, 
     .  fric2,fric3,fric4,bignum,fdat,iseg,fxis,fyis,fzis,ss,tt, 
     .  ilbsv,stfk,frc,numnp,npc,pld,lcfst,lcfdt,temp,temp_bot, 
     .  temp_top,isurface) 
c 
c****************************************************************** 
c|  LIVERMORE SOFTWARE TECHNOLOGY CORPORATION  (LSTC)             | 
c|  ------------------------------------------------------------  | 
c|  COPYRIGHT © 1987-2007 JOHN O.  HALLQUIST, LSTC                 | 
c|  ALL RIGHTS RESERVED                                           | 
c****************************************************************** 
c 
c     user subroutine for interface friction control 
c 
c     note:  LS-DYNA uses an internal numbering system to 
c            accomodate arbitrary node numbering.   to access 
c            information for user node n, address array location m, 
c            m=lqf(n,1).  to obtain user node number, n, 
c            corresponding to array address m, set n=lqfinv(m,1) 
c 
c     arguments: 
c 
c          nosl       =number of sliding interface 
c          time       =current solution time 
c          ncycle     =ncycle number 
c          dt2        =time step size at n+1/2 
c          insv       =slave node array where the nodes are stored 
c                      in ls-dyna3d internal numbering.  User numbers 
c                      are given by function: lqfinv(insv(ii),1) 
c                      for slave node ii. 
c          areas(ii)  =slave node area (interface types 5&10 only) for 
c                      slave node ii 
c          xs(ii)     =x-coordinate slave node ii (projected) 
c          ys(ii)     =y-coordinate slave node ii (projected) 
c          zs(ii)     =z-coordinate slave node ii (projected) 
c          lsv(ii)    =master segment number for slave node ii 
c          ix1(ii), ix2(ii), ix3(ii), ix4(ii) 
c                     =master segment nodes in ls-dyna3d internal 
c                      numbering for slave node ii
APPENDIX G 
c          aream(ii)  =master segment area for slave node ii. 
c          xx1(ii,4)  =x-coordinates master surface (projected) for 
c                      slave node ii 
c          xx2(ii,4)  =y-coordinates master surface (projected) for 
c                      slave node ii 
c          xx3(ii,4)  =z-coordinates master surface (projected) for 
c                      slave node ii 
c          stfn       =slave node penalty stiffness 
c          stf        =master segment penalty stiffness 
c          fni        =normal force 
c          dx,dy,dz   =relative x,y,z-displacement between slave node and 
c                      master surface.  Multipling by fdt2 defines the 
c                      relative velocity. 
c          n1,n2,n3   =x,y, and z components of master segments normal 
c                      vector 
c 
c*********************************************************************** 
c       frictional coefficients defined for the contact interface 
c 
c          fric1      =static friction coefficient 
c          fric2      =dynamic friction coefficient 
c          fric3      =decay constant 
c          fric4      =viscous friction coefficient (setting fric4=0 
c                      turns this option off) 
c 
c*********************************************************************** 
c 
c          bignum     =0.0 for one way surface to surface and 
c                      for surface to surface, and 1.e+10 for nodes 
c                      to surface contact 
c          ninput     =number of variables input into ua 
c          ua(*)      =users' array, first ninput locations 
c                      defined by user.  the length of this 
c                      array is defined on control card 10. 
c                      this array is unique to interface nosl. 
c 
c          side       ='master' for first pass.  the master 
c                       surface is the surface designated in the 
c                       input 
c                     ='slave' for second pass after slave and 
c                      master surfaces have be switched for 
c                      the type 3 symmetric interface treatment. 
c 
c          iisv5      =an array giving the pointers to the active nodes 
c                      in the arrays. 
c 
c          niisv5     =number of active nodes 
c 
c          fdat       =contact history data array 
c          iseg       =contact master segment from previous step. 
c          fxis       =slave node force component in global x dir. 
c                      to be updated to include friction 
c          fyis       =slave node force component in global y dir. 
c                      to be updated to include friction 
c          fzis       =slave node force component in global z dir. 
c                      to be updated to include friction 
c          ss(ii)     =s contact point (-1 to 1) in parametric coordinates 
c                      for slave node ii. 
c          tt(ii)     =t contact point (-1 to 1) in parametric coordinates 
c                      for slave node ii. 
c          ilbsv(ii)  =pointer for node ii into global arrays. 
c          stfk(ii)   =penalty stiffness for slave node ii which was used 
c                      to compute normal interface force. 
c          frc(1,lsv(ii)) 
c                    =Coulomb friction scale factor for segment lsv(ii) 
c          frc(2,lsv(ii))
APPENDIX G 
c                    =viscous friction scale factor for segment lsv(ii) 
c 
c*********************************************************************** 
c       parameters for a coupled thermal-mechanical contact 
c 
c          numnp      = number of nodal points in the model 
c          npc        = load curve pointer 
c          pld        = load curve (x,y) data 
c          lcfst(nosl)= load curve number for static coefficient of 
c                       friction versus temperture for contact 
c                       surface nosl 
c          lcfdt(nosl)= load curve number for dynamic coefficient of 
c                       friction versus temperture for contact 
c                       surface nosl 
c          temp(j)    = temperature for node point j 
c          temp_bot(j)= temparature for thick thermal shell bottom 
c                       surface 
c          temp_top(j)= temparature for thick thermal shell top 
c                       surface 
c          numsh12    = number of thick thermal shells 
c          itopaz(1)  = 999 ==> thermal-mechanical analysis 
c          isurface   = thick thermal shell surface pointer 
c 
c***********************************************************************
APPENDIX H 
APPENDIX H:  User Defined 
Thermal Material Model 
The addition of a thermal user material routine into LS-DYNA is fairly straightforward.  
The thermal user material is controlled using the keyword *MAT_THERMAL_USER_-
DEFINED, which is described at the appropriate place in the manual.  
The  thermal  user  material  can  be  used  alone  or  in  conjunction  with  any  given 
mechanical  material  model  in  a  coupled  thermal-mechanical  solution.    A  heat-source 
can  be  included  and  the  specific  heat  updated  so  that  it  possible  to  model  e.g.    phase 
transformations including melt energy. 
If  for  the  same  part  (shell  or  solid  elements)  both  a  thermal  and  mechanical  user 
material  model  is  defined  then  the  two  user  material  models  have  (optionally)  read 
access  to  each  other’s  history  variables.    If  the  integration  points  of  the  thermal  and 
mechanical elements not are coincident then interpolation or extrapolation is used when 
reading history variables.  Linear interpolation or extrapolation using history data from 
the  two  closest  integration  points  is  used  in  all  cases  except  when  reading  history 
variables  from  the  thick  thermal  shell  (THSHEL = 1  on  *CONTROL_SHELL).    For  the 
latter thermal shell, the shape functions of the element are used for the interpolation or 
extrapolation. 
The  thermal  user  materials  are  thermal  material  types  11-15.    These  thermal  user 
material subroutines are defined in file dyn21.f as subroutines thumat11, … , thumat15.  
The  latter  subroutines  are  called  from  the  subroutine  thusrmat.    The  source  code  of 
subroutine thusrmat is also in file dyn21.f.  Additional useful information is available in 
the  comments  of  subroutines  thusrmat,  thumat12,  and  umat46  that  all  reside  in  the 
source file dyn21.f 
Thermal history variables 
Thermal history variables can be used by setting NVH greater that 0.  Thermal history 
variables are output to the tprint file, see *DATABASE_TPRINT. 
Interchange of history variables with mechanical user material 
In a coupled thermo-mechanical solution there is for each mechanical shell, thick shell, 
or  solid  element  a  corresponding  thermal  element.    A  pair  consisting  of  a  mechanical 
and a corresponding thermal element both have integration points and possibly history 
variables.    The  mechanical  and  thermal  elements  do  not  necessarily  have  the  same 
number of integration points.
APPENDIX H 
By setting IHVE to 1, a thermal user material model can read, but not write, the history 
variables from a mechanical user material model and vice versa.  
If the locations of the points where the history variables are located differ between the 
mechanical  and  thermal  element  differ  interpolation  or  extrapolation  is  used  to 
calculate  the  history  value.    More  information  is  available  in  the  comments  to  the 
subroutines thusrmat and thumat11. 
Limitations: 
Currently there are a few limitations of the thermal user material implementation.  LS-
DYNA  will  in  most  cases  give  an  appropriate  warning  or  error  message  when  such  a 
limit is violated.  The limitations include: 
1.  Option  IHVE.EQ.1  is  only  supported  for  a  limited  range  of  mechanical 
elements: 
a)  Solid elements: ELFORM = 1, 2, 10, 13. 
b)  Shell elements: ELFORM = 2, 3, 4, 16.  Note that user-defined integration 
rules are not supported. 
2.  Thermal history variables limitations: 
a)  Thermal history variables are not output to d3plot. 
3.  The thermal solver includes not only the plastically dissipated energy as a heat 
source but also wrongly the elastic energy.  The latter however is in most cases 
not of practical importance. 
Example source code: 
Example  source  code  for  thermal  user  material  models  is  available  in  thumat11  and 
thumat12 as well as in umat46.  Note that there is space for up to 64 material parameters 
in r_matp (material parameter array) but only 32 can be read in from the *MAT_THER-
MAL_USER_DEFINED card.  The material parameters in r_matp(i), i = 41-64, which are 
initially set to 0.0, may be used by the user to store additional data.  
Subroutine crvval evaluates load curves.  Note that when using crvval the load curves 
are first re-interpolated to 100 equidistant points.  See Appendix A for more information 
on subroutine crvval. 
Following  is  a  short  thermal  user  material  model.    The  card  format  is  in  this  case,  if 
enabling orthotropic conduction, and with sample input in SI-units:
Card 1 
1 
Variable 
MID 
2 
RO 
3 
MT 
4 
5 
6 
7 
8 
LMC 
NVH 
AOPT 
IORTHO 
IHVE 
Type 
21 
7800.0 
12.0 
6.0 
3.0 
0.0 
1.0 
0.0 
  Card 2 
Variable 
1 
XP 
2 
YP 
3 
ZP 
4 
A1 
5 
A2 
6 
A3 
7 
8 
Type 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
  Card 3 
Variable 
1 
D1 
2 
D2 
3 
D3 
Type 
0.0 
0.0 
0.0 
4 
5 
6 
7 
8 
  Card 4 
Variable 
1 
C1 
2 
C2 
3 
C3 
4 
HC 
5 
6 
7 
8 
HSRC 
HCFAC 
Type 
25.0 
25.0 
20.0 
470.0 
11.0 
12.0 
  VARIABLE   
DESCRIPTION
C1-C3 
HC 
HSRC 
Heat conduction in 11, 22, and 33 direction of material coordinate 
system. 
Heat capacity 
Load curve ID of load curve giving a heat source output (W/m3)
as a function of time. 
HCFAC 
Load curve ID of load curve giving a scaling of the heat capacity
as function of time.
APPENDIX H 
The source code is: 
      subroutine thumat12(c1,c2,c3,cvl,dcvdtl,hsrcl,dhsrcdtl, 
     1     hsv,hsvm,nmecon,r_matp,crv, 
     2     nel,nep,iep,eltype,dt,atime,ihsrcl) 
      character*(*) eltype 
      dimension hsv(*),hsvm(*),r_matp(*),crv(101,2,*) 
      include 'iounits.inc' 
c 
c     Thermal user-material number 12. 
c 
c     See comments at the beginning of subroutine thusrmat 
c     for instructions. 
c 
c     Example: isotropic/orthotropic material with k1=P1 and 
c     cvl=P2 for solid and shell elements including optional 
c     change of heat capacity and a heat source, both functions 
c     of time input as load curves. 
c 
c     Print out some info on start-up, use material parameter 64 
c     as a flag. 
      if(nint(r_matp(64)).eq.0) then 
         r_matp(64)=1. 
         write( *,1200)  (r_matp(8+i),i=1,6) 
         write(iohsp,1200) (r_matp(8+i),i=1,6) 
         write(59,1200) (r_matp(8+i),i=1,6) 
      endif 
c 
c     Calculate response 
      c1=r_matp(8+1) 
      c2=r_matp(8+2) 
      c3=r_matp(8+3) 
      cvl=r_matp(8+4) 
      dcvdtl=0.0 
      eid=nint(r_matp(8+6)) 
      if(nint(eid).gt.0) then 
         call crvval(crv,eid,atime,cvlfac,tmp1) 
         cvl=cvl*cvlfac 
         dcvdtl=0.0 
      endif 
c 
c     If flux or time step calculation then we are done. 
      if(eltype.eq.'soliddt'.or.eltype.eq.'flux'.or. 
     .     eltype.eq.'shelldt') return 
      eid=nint(r_matp(8+5)) 
      if(nint(eid).gt.0) then 
         ihsrcl=1 
         call crvval(crv,eid,atime,hsrcl,tmp1) 
         dhsrcdtl=0.0 
      endif 
c 
c     Update history variables 
      hsv(1)=cvl 
      hsv(2)=atime 
      hsv(3)=hsv(3)+1.0 
c 
c     Done 
      return 
 1200 format(/'This is thermal user defined material #12.  '/ 
     1        /' Material parameter c1-c3       : ',3E10.3 
     2        /' Material parameter hc          : ',E10.3 
     3        /' Heat source load curve         : ',F10.0 
     4        /' hc scale factor load curve     : ',F10.0 
     5        /' Thermal History variable 1     : cv' 
     6        /' Thermal History variable 2-3   : Dummy'/)
return 
      end
APPENDIX H
APPENDIX I 
APPENDIX I:  Occupant Simulation 
Including the Coupling to the 
CAL3D and MADYMO programs 
INTRODUCTION 
LS-DYNA is coupled to occupant simulation codes to generate solutions in automotive 
crashworthiness  that  include  occupants  interacting  with  the  automotive  structure.    In 
such  applications  LS-DYNA  provides  the  simulation  of  the  structural  and  deformable 
aspects of the model and the OSP (Occupant Simulation Program) simulates the motion 
of  the  occupant.    There  is  some  overlap  between  the  two  programs  which  provides 
flexibility  in  the  modeling  approach.    For  example,  both  the  OSP  and  LS-DYNA  have 
the capability of modeling seat belts and other deformable restraints.  The advantage of 
using  the  OSP  is  related  to  the  considerable  databases  and  expertise  that  have  been 
developed in the past for simulating dummy behavior using these programs. 
The development of the interface provided LSTC a number of possible approaches.  The 
approach selected is consistent with the LSTC philosophy of providing the most flexible 
and  useful  interface  possible.    This  is  important  because  the  field  of  non-linear 
mechanics  is  evolving  rapidly  and  techniques  which  are  used  today  are  frequently 
rendered obsolete by improved methodologies and lower cost computing which allows 
more  rigorous  techniques  to  be  used.    This  does  make  the  learning  somewhat  more 
difficult as there is not any single procedure for performing a coupling. 
One  characteristic  of  LS-DYNA  is  the  large  number  of  capabilities,  particularly  those 
associated  with  rigid  bodies.    This  creates  both  an  opportunity  and  a  difficulty:    LS-
DYNA3D  has  many  ways  approximating  different  aspects  of  problems,  but  they  are 
frequently  not  obvious  to  users  without  considerable  experience.    Therefore,  in  this 
Appendix we emphasize modeling methods rather than simply listing capabilities. 
THE LS-DYNA/OCCUPANT SIMULATION PROGRAM LINK 
Coupling  between  the  OSP  and  LS-DYNA  is  performed  by  combining  the  programs 
into a single executable.  In the case of CAL3D, LS-DYNA calls CAL3D as a subroutine, 
but in the case of MADYMO, LS-DYNA is called as a subroutine.  The two programs are 
then  integrated  in  parallel  with  the  results  being  passed  between  the  two  until  a  user 
defined termination time is reached. 
The OSP and LS-DYNA have different approaches to the time integration schemes.  The 
OSP time integrators are based on accurate implicit integrators which are valid for large 
time  steps  which  are  on  the  order  of  a  millisecond  for  the  particular  applications  of
APPENDIX I 
interest  here.    An  iterative  solution  is  used  to  insure  that  the  problem  remains  in 
equilibrium.    The  implicit  integrators  are  extremely  good  for  smoothly  varying  loads, 
however, sharp nonlinear pulses can introduce considerable error.  An automatic time 
step  size  control  which  decreases  the  time  step  size  quickly  restores  the  accuracy  for 
such  events.    The  LS-DYNA  time  integrator  is  based  on  an  explicit  central  difference 
scheme.  Stability requires that the time step size be less than the highest frequency in 
the system.  For a coarse airbag mesh, this number is on the order of 100 microseconds 
while an actual car crash simulation is on the order of 1 microsecond.  The smallest LS-
DYNA  models  have  at  least  1,000  elements.    Experience  indicates  that  the  cost  of  a 
single LS-DYNA time step for a small model is at least as great as the cost of a time step 
in  the  OSP.    Therefore,  in the  coupling,  the  LS-DYNA  time  step  is  used  to  control  the 
entire  simulation  including  the  OSP  part.    This  approach  has  negligible  cost  penalties 
and avoids questions of stability and accuracy that would result by using a subcycling 
scheme between the two programs.   
LS-DYNA has a highly developed rigid body capability which is used in different parts 
of  automobile  crash  simulation.    In  particular,  components  such  as  the  engine  are 
routinely  modeled  with  rigid  bodies.    These  rigid  bodies  have  been  modified  so  that 
they form the basis of the coupling procedure in LS-DYNA to the OSP. 
Please  contact  the  LSTC  technical  support  team  (support@lstc.com)  for  instructions  to 
download and run LS-DYNA executables coupled with Madymo. 
AIRBAG MODELING 
Modeling  of  airbags  is  accomplished  by  use  of  shell  or  membrane  elements  in 
conjunction  with  a  control  volume    and  possibly  a  single 
surface contact algorithm to eliminate interpenetrations during the inflation phase .  The contact types showing an “a” in front are most suited for 
airbag analysis.  Current recommended material types for the airbags are: 
1. 
2. 
3. 
*MAT_ELASTIC (Type 1, Elastic) 
*MAT_COMPOSITE_DAMAGE  (Type  22,  layered  orthotropic  elastic  for 
composites) 
*MAT_FABRIC (Type 34, fabric model for folded airbags) 
Model  34  is  a  “fabric”  model  which  can  be  used  for  flat  bags.    As  a  user  option  this 
model may or may not support compression. 
The elements which can be used are as follows: 
1.  Belytschko-Tsay  quadrilateral  with  1  point  quadrature.    This  element  behaves 
rather well for folded and unfolded cases with only a small tendency to hour-
APPENDIX I 
glass.  The element tends to be a little stiff.  Stiffness form hourglass control is 
recommended. 
2.  Belytschko-Tsay  membrane.    This  model is  softer  than  the  normal  Belytschko-
Tsay  element  and  can  hourglass  quite  badly.    Stiffness  form  hourglass  is  rec-
ommended.  As a better option, the fully integrated Belytschko-Tsay membrane 
element can be chosen. 
3.  C0 Triangular element.  The C0 triangle is very good for flat bag inflation and 
has no tendency to hourglass. 
4.  The  best  choice  is  a  specially  developed  airbag  membrane  element  with 
quadrilateral  shape.    This  is  an  automatic  choice  when  the  fabric  material  is 
used. 
As an airbag inflates, a considerable amount of energy is transferred to the surrounding 
air.    This  energy  transfer  decreases  the  kinetic  energy  of  the  bag  as  it  inflates.    In  the 
control volume logic, this is simulated either by using either a mass weighted damping 
option or a back pressure on the bag based on a stagnation pressure.  In both cases, the 
energy  that  is  absorbed  is  a  function  of  the  fabric  velocity  relative  to  a  rigid  body 
velocity  for  the  bag.    For  the  mass  weighted  case,  the  damping  force  on  a  node  is 
proportional  to  the  mass  times  the  damping  factor  times  the  velocity  vector.    This  is 
quite  effective  in  maintaining a  stable  system,  but  has  little  physical  justification.    The 
latter approach using the stagnation pressure method estimates the pressure needed to 
accelerate the surrounding air to the speed of the fabric.  The formula for this is: 
𝑃 = Area × 𝛼 × [(𝑉⃗⃗⃗⃗⃗𝑖 − 𝑉⃗⃗⃗⃗⃗𝑐𝑔) ⋅ 𝑛̂]
This formula accomplishes a similar function and has a physical justification.  Values of 
the damping factor, 𝛼, are limited to the range of 0 to 1, but a value of 0.1 or less is more 
likely to be a good value. 
COMMON ERRORS 
1. 
Improper airbag inflation or no inflation. 
The  most  common  problem  is  inconsistency  in  the  units  used  for  the  input 
constants.  An inflation load curve must also be specified.  The normals for the 
airbag segments must all be consistent and facing outwards.  If a negative vol-
ume results, this can sometimes be quickly cured by using the “flip” flag on the 
control volume definition to force inward facing normals to face outwards. 
2.  Excessive airbag distortions. 
Check the material constants.  Triangular elements should have less distortion 
problems  than  quadrilaterals.    Overlapped  elements  at  time  zero  can  cause
APPENDIX I 
locking to occur in the contact leading to excessive distortions.  The considera-
ble  energy  input  to  the  bag  will  create  numerical  noise  and  some  damping  is 
recommended to avoid problems. 
3.  The dummy passes through the airbag. 
A  most  likely  problem  is  that  the  contacts  are  improperly  defined.    Another 
possibility  is  that  the  models  were  developed  in  an  incompatible  unit  system.  
The extra check for penetration flag if set to 1 on the contact control cards vari-
able PENCHK in the *CONTACT_...  definitions may sometimes cause nodes to 
be prematurely released due to the softness of the penalties.  In this case the flag 
should be turned off.  
4.  The OSP fails to converge. 
This  may  occur  when  excessively  large  forces  are  passed  to  the  OSP.    First, 
check  that  unit  systems  are  consistent  and  then  look  for  improperly  defined 
contacts in the LS-DYNA input. 
5.  Time step approaches zero. 
This is almost always in the airbag.  If elastic or orthotropic (*MAT_ELASTIC or 
*MAT_COMPOSITE material 1 or 22) is being used, then switch to fabric mate-
rial *MAT_FABRIC which is less time step size sensitive and use the fully inte-
grated  membrane  element.    Increasing  the  damping  in  the  control  volume 
usually  helps  considerably.    Also,  check  for  “cuts”  in  the  airbag  where  nodes 
are  not  merged.    These  can  allow  elements  to  deform  freely  and  cut  the  time 
step to zero.
APPENDIX J 
APPENDIX J:  Interactive 
Graphics Commands 
Only the first four or less characters of command are significant.  These commands are 
available in the interactive phase of LS-DYNA.  The interactive graphics are available by 
using the “SW5.” command after invoking the Ctrl-C interrupt.  The MENU command 
brings up a push button menu.  Only available in Unix and Linux. 
ANIMATE 
Animate saved sequence, stop with switch 1. 
BACK 
BGC 
BIP 
CENTER 
CL 
CMA 
COLOR 
Return  to  previous  display  size  after  zoom,  then  list 
display attributes. 
Change display background color RGB proportions BGC 
<red> <green> <blue>. 
Select beam integration point for contour; BIP <#>. 
Center model, center on node, or center with mouse, i.e., 
center cent <value> or cent gin. 
Classification  labels  on  display;  class  commercial_in_
confidence. 
Color materials on limited color displays. 
Set or unset shaded coloring of materials. 
CONTOUR 
View  with  colored  contour  lines;  contour < component 
#> < list mat #>; see TAURUS manual. 
COOR 
COP 
CR 
CUT 
CX 
CY 
CZ 
Get node information with mouse. 
Hardcopy of display on the PC copy < laserj paintj tekcol 
coljet or epson>. 
Restores cutting plane to default position. 
Cut away model outside of zoom window; use mouse to 
set zoom window size. 
Rotate slice plane at zmin about x axis. 
Rotate slice plane at zmin about y axis. 
Rotate slice plane at zmin about z axis.
APPENDIX J 
DIF 
DISTANCE 
Change  diffused  light  level  for  material;  DIF < mat  #,  -1 
for all > <value>. 
Set  distance  of  model  from  viewer;  DIST < value  in 
normalized model dimensions>. 
DMATERIALS 
Delete  display  of  material 
DMAT < ALL or list of numbers>. 
in  subsequent  views;  
DRAW 
DSCALE 
DYN 
ELPLT 
END 
ESCAPE 
EXECUTE 
FCL 
FOV 
FRINGE 
Display outside edges of model. 
Scale current displacement from initial shape. 
After using TAURUS command will reset display to read 
current DYNA3D state data. 
Set or unset element numbering in subsequent views. 
Delete display and return to execution. 
Escapes from menu pad mode. 
Return to execution and keep display active. 
Fix or unfix current contour levels. 
Set display field of view angle; FOV < value in degrees>. 
View  with  colored  contour  fringes;  fringe < component 
#> < list mat #>; see TAURUS manual. 
GETFRAME 
Display a saved frame; GETF < frame #>. 
HARDWARE 
Hardware mode; workstation hardware calls are used to 
draw, move and color model; repeat command to reset to 
normal mode. 
HELP 
HZB 
LIMIT 
MAT 
Switch on or off hardware zbuffer for a subsequent view, 
draw  or  contour  command;  rotations  and  translations 
will be in hardware. 
Set range of node numbers subsequent views; limit < first 
node #> < last node #>. 
Re-enable display of deleted materials mat < all or list of 
numbers>.
MENU 
MOTION 
MOV 
NDPLT 
APPENDIX J 
Button menu pad mode. 
Motion  of  model  through  mouse  movement  or  use  of  a 
dial box.  The left button down enables translation in the 
plane,  middle  button  rotation  about  axes  in  the  plane; 
and with right button down in the out of plane axis; left 
and middle button down quit this mode. 
Drag picked part to new position set with mouse. 
Set or unset node numbering in subsequent views. 
NOFRAME 
Set and unset drawing of a frame around the picture. 
PAUSE 
Animation display pause in seconds 
PHS2 or THISTORY 
Time history plotting phase.  Similar to LS-TAURUS. 
PICK 
POST 
QUIT 
RANGE 
RAX 
RAY 
RAZ 
RESTORE 
Get element information with mouse. 
Enable or disable postscript mode on the PC and eps file 
is  written  as  picture  is  drawn;  remove  eofs  and  init-
graphics for eps use. 
Same as execute. 
Set  fix  range  for  contour  levels;  range  <minvalue> 
<maxvalue>. 
Reflect  model  about  xy  plane;  restore  command  will 
switch-off reflections. 
Reflect  model  about  yz  plane;  restore  command  will 
switch-off reflections. 
Reflect  model  about  zx  plane,  restore  command  will 
switch-off reflections. 
Restores  model  to  original  position,  also  switches  off 
element  and  node  numbers,  slice  capper,  reflections  and 
cut model. 
RETURN 
Exit. 
RGB 
RX 
Change  color  red  green  blue  element < mat  #>  <red> 
<green> <blue>. 
Rotate model about x axis.
APPENDIX J 
RY 
RZ 
SAVE 
SEQUENCE 
SHR 
SIP 
SLICE 
SNORMAL 
SPOT 
TAURUS 
TRIAD 
TSHELL 
TV 
TX 
TY 
TZ 
V 
VECTOR v or d 
ZB 
ZIN 
Rotate model about y axis. 
Rotate model about z axis. 
Set or unset saving of display for animation. 
Periodic  plot  during  execution;  SEQ  <#  of  cy-
cles > <commands> EXE. 
Shrink  element  facets  towards  centroids  in  subsequent 
views, shrink <value>. 
Select shell integration point for contour; SIP <#>. 
Slice  model  a  z-minimum  plane;  slice < value 
in 
normalized  model  dimension > this  feature  is  removed 
after using restore.  Slice enables internal details for brick 
elements  to  be  used  to  generate  new  polygons  on  the 
slice plane. 
Set or unset display of shell direction normals to indicate 
topology order. 
Draw node numbers on model spot < first #> < last # for 
range>. 
LS-DYNA  database,  TAU < state  #>,  or  state < state  #>, 
reads LS-TAURUS file to extract previous state data. 
Set or unset display of axis triad. 
Set  or  unset  shell  element  thickness  simulation  in 
subsequent views. 
Change display type. 
Translates model along x axis. 
Translates model along y axis. 
Translates model along z axis. 
Display model using painters algorithm. 
View with vector arrows of velocity or displacement; <v> 
or <d>. 
Switch  on  or  off  zbuffer  algorithm  for  subsequent  view; 
or draw commands. 
Zoom in using mouse to set display size and position.
ZMA 
ZMI 
ZOUT 
APPENDIX J 
Set position of zmax plane; ZMAX < value in normalized 
model dimensions>. 
Set  position of  zmin  plane;  ZMIN < value  in  normalized 
model dimensions>. 
Zoom out using mouse to set displays size expansion and 
position.
APPENDIX K 
APPENDIX K:  Interactive 
Material Model Driver 
INTRODUCTION 
The  interactive  material  model  driver  in  LS-DYNA  allows  calculation  of  the  material 
constitutive  response  to  a  specified  strain  path.    Since  the  constitutive  model 
subroutines  in  LS-DYNA  are  directly  called  by  this  driver,  the  behavior  of  the 
constitutive model is precisely that which can be expected in actual applications.  In the 
current  implementation  the  constitutive  subroutines  for  both  shell  elements  and  solid 
elements can be examined. 
INPUT DEFINITION 
The  material  model  driver  is  invoked  when  no  *NODE  or  *ELEMENT  commands  are 
present  in  a  standard  LS-DYNA  input  file.   The  number  of  material  model  definitions 
should  be  set  to  one,  the  number  of  load  curves  should  be  nine,  and  the  termination 
time to the desired length of the driver run.  The complete state dump interval as given 
in  *DATABASE_BINARY_D3PLOT  serves  as  the  time  step  to  be  used  in  the  material 
model  driver  run.    Plotting  information  is  saved    in  core  for  the  interactive  plotting 
phase. 
The input deck typically consists only of *KEYWORD, *DATABASE_BINARY_D3PLOT, 
*CONTROL_TERMINATION,  one  each  of  *PART/*MAT/*SECTION,    and  nine  load 
curves (*DEFINE_CURVE) describing the strain path.  These nine curves define the time 
history of the displacement gradient components shown in Table 54-1. 
The  velocity  gradient  matrix,  Lij,  is  approximated  by  taking  the  time  derivative  of  the 
components in Table 54-1.  If these components are considered to form a tensor Sij , then 
𝐿𝑖𝑗(𝑡) =
𝑆𝑖𝑗(𝑡) − 𝑆𝑖𝑗(𝑡𝑘−1)
(𝑡 − 𝑡𝑘)
and the strain rate tensor is defined as  
and the spin tensor as 
𝑑𝑖𝑗 =
𝐿𝑖𝑗 + 𝐿𝑖𝑗
𝜔𝑖𝑗 =
𝐿𝑖𝑗 − 𝐿𝑖𝑗
APPENDIX K 
Load Curve Number 
Component Definition 
1 
2 
3 
4 
5 
6 
7 
8 
9 
∂𝑢
∂𝑥
∂𝑣
∂𝑦
∂𝑤
∂𝑧
∂𝑢
∂𝑦
∂𝑣
∂𝑥
∂𝑢
∂𝑧
∂𝑤
∂𝑥
∂𝑣
∂𝑧
∂𝑤
∂𝑦
Table 54-1.   Load Curve Definitions versus Time 
INTERACTIVE DRIVER COMMANDS 
After  reading  the  input  file  and  completing  the  calculations,  LS-DYNA  gives  a 
command prompt to the terminal.  A summary of the available interactive commands is 
given below.  An on-line help package is available by typing HELP.  Only available in 
Unix and Linux. 
ACCL 
Scale all abscissa data by f.  Default is f = 1. 
ASET amin omax 
Set  min  and  max  values  on  abscissa  to  amin  and 
amax,  respectively.    If  amin = amax = 0,  scaling  is 
automatic. 
CHGL n  
Change 
prompts for new label. 
label  for  component  n. 
  LS-DYNA
APPENDIX K 
CONTINUE 
Re-analyze material model. 
CROSS c1 c2 
Plot component c1 versus c2. 
ECOMP 
Display  component  numbers  on  the  graphics  dis-
play: 
EQ.1:  x-stress, 
EQ.2:  y-stress, 
EQ.3:  z-stress, 
EQ.4:  xy-stress, 
EQ.5:  yz-stress, 
EQ.6:  zx-stress, 
EQ.7:  effective plastic strain, 
EQ.8:  pressure, 
EQ.9:  von Mises (effective) stress, 
EQ.10: 1st principal deviatoric stress, 
EQ.11: 2nd principal deviatoric stress, 
EQ.12: 3rd principal deviatoric stress, 
EQ.13: maximum shear stress, 
EQ.14: 1st principal stress, 
EQ.15: 2nd principal stress, 
EQ.16: 3rd principal stress, 
EQ.17: ln (v ⁄ v0), 
EQ.18: relative volume, 
EQ.19: v0 ⁄ v - 1.0, 
EQ.20: 1st history variable, 
EQ.21: 2nd history variable. 
Adding  100  or  400  to  component  numbers  1-16 
yields strains and strain rates, respectively. 
FILE name 
Change pampers filename to name for printing. 
GRID 
NOGRID 
Graphics displays will be overlaid by a grid of or-
thogonal lines. 
Graphics displays will not be overlaid by a grid of 
orthogonal lines. 
OSCL 
Scale all ordinate data by f.  Default is f = 1. 
OSET omin omax 
Set  min  and  max  values  on  ordinate  to  omin  and 
omax, respectively.  If omin = omax = 0, scaling is 
automatic.
APPENDIX K 
PRINT 
Print plotted time history data into file “pampers.”  
Only  data  plotted  after  this  command  is  printed.  
File  name  can  be  changed  with  the  “file”  com-
mand. 
QUIT, END, T 
Exit the material model driver program. 
RDLC m n r1 z1 ...  rn zn  Redefine  load  curve  m  using  n  coordinate  pairs 
(r1,z1) (r2,z2),...(rn,zn). 
TIME c 
TV n 
Plot component c versus time. 
Use  terminal  output  device  type  n.    LS-DYNA 
provides a list of available devices. 
Presently, the material model drive is implemented for solid and shell element material 
models.  The driver does not yet support material models for beam elements.  
Use  the  keyword  *CONTROL_MPP_MATERIAL_MODEL_DRIVER  and  run  the  input 
deck only on one processor if a distributed memory executable (MPP) is used.
APPENDIX L 
APPENDIX L:  VDA Database 
VDA  surfaces  describe  the  surface  of  geometric  entities  and  are  useful  for  the 
simulation  of  sheet  forming  problems.    The  German  automobile  and  automotive 
supplier  industry  (VDA)  has  defined  the  VDA  guidelines  [VDA  1987]  for  a  proper 
surface definition used for the exchange of surface data information.  In LS-DYNA, this 
format can be read and used directly.  Some files have to be provided for proper linkage 
to the motion of the correlation parts/materials in LS-DYNA. 
Linking is performed via names.   To these names surfaces are attached, which  in turn 
can be linked together from many files externally to LS-DYNA.  Thus, arbitrary surfaces 
can  be  provided  by  a  preprocessor  and  then  can  be  written  to  various  files.    The  so-
called VDA file given on the LS-DYNA execution line via V = vda contains references to 
all  other  files.    It  also  contains  several  other  parameters  affecting  the  treatment  in  the 
contact subroutines; see below. 
The  procedure  is  as  follows.    If  VDA  surfaces  are  to  be  used,  the  file  specified  by vda 
must  have  the  following  form.    The  file  is  free  formatted  with  blanks  as  delimiters.  
Note that the characters “}” and “{” must be separated from the other input by spaces or 
new lines.  The vda file may contain any number of input file specifications of the form: 
file afile bfile { 
alias definitions 
} 
alias definitions 
followed by optional runtime parameters and a final end statement. 
The  file,  afile,  is  optional,  and  if  given  must  be  the  name  of  an  ASCII  input  file 
formatted  in  accordance  with  the  VDA  Surface  Interface  Definitions  as  defined  by  the 
German automobile and automotive supply industry.  bfile is required, and is the name 
of a binary VDA file.  In a first run afile is given and bfile is created.  In any further run, 
if the definitions have not changed, afile can be dropped and only bfile is needed.  The 
purpose of bfile is that it allows for much faster initialization if the same VDA surfaces 
are to be used in a future LS-DYNA run.   
If  afile  is  given,  bfile  will  always  be  created  or  overwritten.    The  alias  definitions  are 
used  for  linking  to  LS-DYNA  and  between  the  various  surface  definitions  in  the  files 
defined by afile and bfile. 
The alias definitions are of the form 
alias name { el1 el2 ...  eln } 
where  name  is  any  string  of  up  to  12  characters,  and  el1,...,eln  are  the  names  of  VDA 
elements as specified in afile.  The list of elements can be empty, in which case all the 
SURF and FACE VDA elements in afile will be used.  Care should be taken to ensure 
that  the  alias  name  is  unique,  not  only  among  the  other  aliases,  but  among  the  VDA
APPENDIX L 
offset  10  5  0  0  1
goffset  alias  die  1  2  1  5  0  0  1
{  previous  alias  dieold  }
vw
die
P = (1,2,1)
zoffset = 1
woffset = 5
element 10
(a)
zoffset = 1
poffset = 5
dieold
(b)
Figure  55-1.    (a)  a  schematic  illustration  of  offset  version  1,  and  (b)  is  a
schematic illustration of offset version 2. 
element names in afile.  This collection of VDA elements can later be indicated by the 
alias name.  In particular, name may appear in later alias definitions. 
Often  it  is  required  that  a  punch  or  die  be  created  by  a  simple  offset.    This  can  be 
achieved  in  the  vda  files  in  two  ways,  either  on  VDA  elements  directly,  or  on  parts 
defined by aliases.  This feature offers great capability in generating and using surface 
data information. 
Offset Version 1 
As  an  option,  the  keyword  offset  may  appear  in  the  alias  list  which  allows  a  new 
surface to be created as a normal offset (plus translation) of a VDA element in the file.  
The  keyword  offset  my  be  applied  to  VDA  elements  only,  not  aliases.    The  usage  of 
offset follows the form 
offset elem normal x y z 
where normal is the amount to offset the surface along the normal direction, and x,y,z 
are  the  translations  to  be  applied.    The  default  normal  direction  is  given  by  the  cross 
product of the local u and v directions on the VDA surface, taken in that order.  normal 
can be negative.   
Offset Version 2 
Frequently, it is convenient to create a new alias name by offsetting and translating an 
existing name.  The keyword goffset provides this function: 
goffset alias name xc yc zc normal x y z { previous alias name }
where normal, x, y, and z are defined as in the offset keyword.  A reference point xc, yc, 
and  zc  defines  a  point  in  space  which  determines  the  normal  direction  to  the  VDA 
surface, which is a vector from the origin to P(xc,yc,zc).  See example below. 
APPENDIX L 
Finally, several parameters affecting the VDA surface iteration routines can be reset in 
the file vda.  These parameters, and their default values in square brackets [ ], are: 
gap [5.0] 
track [2.0] 
track2 [5.0] 
ntrack [4] 
The  maximum  allowable  surface  gap  to  be  filled  in  during  the 
iterations.  Points following the surface will effectively extend the edg-
es of surfaces if necessary to keep them from falling through cracks in 
the  surface  smaller  than  this.    This  number  should  be  set  as  small  as 
possible while still allowing correct results.  In particular, if your VDA 
surfaces are well formed (having no gaps), this parameter can be set to 
0.0.  The default value is 5.0. 
A  point  must  be  within  this  distance  of  contact  to  be  continually 
tracked.    When  a  point  not  being  tracked  comes  close  to  a  surface,  a 
global search is performed to find the near surface point.  While a point 
is being tracked, iterations are performed every cycle.  These iterations 
are much faster, but if the point is far away it is faster to occasionally do 
the global search.  The default value is 2.0. 
Every  VDA  surface  is  surrounded  by  a  bounding  box.    When  a  global 
search needs to be performed but the distance from a point to this box 
is > track2, the actual global search is not performed.  This will require 
another global search to be performed sooner than if the actual distance 
to the surface were known, but also allows many global searches to be 
skipped.  The default value is 5.0. 
The  number  of  VDA  surfaces  for  which  each  point  maintains  actual 
distance information.  A global lower bound on distance is maintained 
for all remaining surfaces.  Whenever the point moves far enough to vi-
olate  this  global  lower  bound,  all  VDA  surfaces  must  have  the  global 
search performed for them.  Hence, this parameter should be set to the 
maximum number of surfaces that any point can be expected to be near 
at  one  time  (the  largest  number  of  surfaces  that  come  together  at  one 
point).    Setting  ntrack  higher  will  require  more  memory  but  result  in 
faster execution.  If ntrack is too low, performance may be unacceptably 
slow.  The default value is 4.0.
APPENDIX L 
toroid [.01] 
Any surface with opposing edges which are within distance [t] of each 
other is assumed to be cylindrical.  Contacts occurring on one edge can 
pass to the adjacent edge.  The default value is 0.01. 
converge [.01]  When surface iterations are performed to locate the near point, iteration 
is  continued  until  convergence  is  detected  to  within  this  distance  (all 
VDA coordinates are in mm).  The default value is 0.01. 
iterate [8] 
Maximum  number  of  surface  iterations  allowed.    Since  points  being 
tracked  are  checked  every  cycle,  if  convergence  fails  it  will  be  tried 
again  next  cycle,  so  setting  this  parameter  high  does  not  necessarily 
help  much.    On  the  other  hand,  a  point  converging  to  a  crease  in  the 
VDA  surface  (a  crease  between  patches  with  discontinuous  derivative, 
for  example)  may  bounce  back  and  forth  between  patches  up  to  this 
many times, without actually moving.  Hence, this value should not be 
too large.  The default value is 8. 
el_size [t  mx  mn] 
Controls the generation of elements where: 
t =  surface tolerance for mesh generation, 
mx =  maximum element size to generate, 
mn =  minimum element size to generate. 
The default values are [0.25 100.  1.0] 
aspect [s1 s2]  Controls the generation of elements where: 
s1 =  maximum  difference 
in  aspect  ratio  between  elements 
generated in neighboring VDA patches, 
s2 =  maximum aspect ratio for any generated element. 
The default values are [1.5 4.0] 
cp_space [10]  Determines  the  spacing  around  the  boundaries  of  parts  at  which  the 
size  of  elements  is  controlled.    In  the  interior  of  the  part,  the  element 
size is a weighted function of these control points as well as additional 
control points in the interior of the region.  If there are too few control 
points around the boundary, elements generated along or near straight 
boundaries, but between control points, may be too small.  The default 
value is 10. 
meshonly 
The  existence  of  this  keyword  causes  LS-DYNA  to  generate  a  file 
containing the mesh for the VDA surfaces and then terminate. 
onepatch 
The  existence  of  this  keyword  causes  LS-DYNA  to  generate  a  single 
element on each VDA patch.
somepatch [n]  Like onepatch, but generates an element for 1 out of every [n] patches. 
Example for file V = vda.  It contains the following data: 
APPENDIX L 
file vda1 vda1.bin { 
alias die {  
sur0001  
sur0003 
offset fce0006 1.5 0 0 120 
} 
alias holder1 { sur008 } 
} 
file vda2 vda2.bin { 
alias holder2 { sur003 } 
} 
alias holder { holder1 holder2 } 
ntrack 6 
gap 0.5 
end 
Explanation: 
vda1 
This file contains the surfaces/face elements  sur0001,sur0003, fce0006, 
and sur0008. 
alias die face  Combines  the  surface/face  elements  sur0001,  sur0003,  and  the 
offsetted fce0006 to a global surface. 
alias holder1  Defines the surface/face element sur0008 as holder1. 
vda2 
This file contains the surface/face element sur0003. 
alias holder2  Defines the surface/face element sur0003 as holder2. 
alias holder 
Combines  the  surfaces  holder1  and  holder2  into  a  combined  surface 
holder. 
ntrack 6 
For each point the actual distances to 6 VDA surfaces are maintained. 
gap 0.5 
Surface gaps of 0.5mm or less are filled. 
end 
Closes reading of this file.
APPENDIX M 
APPENDIX M:  Commands for 
Two-Dimensional Rezoning 
The rezoner in LS-DYNA contains many commands that can be broken down into the 
following categories: 
•general, 
•termination of interactive rezoning, 
•redefinition of output intervals for data, 
•graphics window controls, 
•graphics window controls for x versus y plots, 
•mesh display options, 
•mesh modifications, 
•boundary modifications, 
•MAZE line definitions, 
•calculation graphics display control parameters, 
•calculation graphics display, 
•cursor commands. 
The use of the rezoner is quite simple.  Commands for rezoning material number n can 
be invoked after the material is specified by the “M n” command.   To view material n, 
the  command  “V”  is  available.    The  interior  mesh  can  be  smoothed  with  the  “S” 
command  and  the  boundary  nodes  can  be  adjusted  after  the  “B”  command  is  used  to 
display  the  part  side  and  boundary  node  numbers.    Commands  that  are  available  for 
adjusting boundary nodes following the “B” command include: 
ER, EZ, ES, VS, BD, ERS, EZS, ESS, VSS, BDS, SLN, SLNS 
Rezoning is performed material by material.  An example is shown. 
Do not include the graphics display type number  when 
setting  up  a  command  file  for  periodic  noninteractive  rezoning.    No  plotting  is  done 
when the rezoner is used in this mode. 
REZONING COMMANDS BY FUNCTION: 
Interactive Real Time Graphics 
SEQ n commands EXE 
Every  n  time  steps  execute  the  graphics  commands 
which follow.  For example the line seq 100 g exe would
APPENDIX M 
General 
C 
FRAME 
HELP 
cause the grid to be updated on the graphics display de-
vice every 100 cycles.  The real time graphics can be ter-
minated by using ctrl-c and typing “sw7.” 
Comment - proceed to next line. 
Frame plots with a reference grid (default). 
Enter  HELP  package  and  display  all  available 
commands.  Description of each command is available in 
the HELP package. 
HELP/commandname 
Do not enter HELP package but print out the description 
on the terminal of the command following the slash. 
LOGO 
NOFRAME 
PHP ans 
RESO nx ny 
TV n 
TR t  
Put  LLNL  logo  on  all  plots  (default).    Retyping  this 
command removes the logo. 
Do not plot a reference grid. 
Print  help  package  -  If  answer  equals  ‘y’  the  package  is 
printed in the high speed printer file. 
Set  the  x  and  y  resolutions  of  plots  to  nx  and  ny, 
respectively.  We default both nx and ny to 1024.   
Use  graphics  output  device  type  n.    The  types  are 
installation  dependent  and  a  list  will  be  provided  after 
this command is invoked. 
At  time  t,  LS-DYNA  will  stop  and  enter  interactive 
rezoning phase. 
Termination of Interactive Rezoning 
F 
FR 
Terminate 
execution phase. 
interactive  phase, 
remap,  continue 
in 
Terminate  interactive  phase,  remap,  write  restart  dump, 
and call exit. 
T or END 
Terminate.
APPENDIX M 
Redefinition of Output Intervals for Data 
PLTI  t 
PRTI  t 
TERM t  
Reset the node and element data dump interval   t. 
Reset the node and element printout interval  t. 
Reset the termination to t. 
Graphics Window Controls 
ESET n 
FF 
FIX 
FSET n  r  z 
GSET r z  l 
GRID 
NOGRID 
SETF r z  r  z  
UNFIX 
UZ a b  l  
Center picture at element n with a  r by  z window.  This 
window  is  set  until  it  is  released  by  the  unfix  command 
or reset with another window. 
Encircle  picture  with  reference  grid  with  tickmarks.  
Default grid is plotted along bottom and left side of pic-
ture. 
Set the display to its current window.  This window is set 
until  it  is  reset  by  the  “GSET,  “FSET”,  or  “SETF”  com-
mands or released by the “UNFIX” command. 
Center  display  at  node  n  with  a  rectangular  Δ𝑟 × Δ𝑧 
window.   This window is  set until it is reset with or the 
“UNFIX” command is typed. 
Center display picture at point (r,z) with square window 
of  width   l.    This  window  is  set  until  it  is  reset  or  the 
“UNFIX” command is typed. 
Overlay  graphics  displays  with  a  grid  of  orthogonal 
lines. 
Do  not  overlay  graphics  displays  with  a  grid  of 
orthogonal lines (default). 
Center  display  at  point  (r,z)  with  a  rectangular  Δ𝑟 × Δ𝑧 
window.  This window is set until it is reset or the “UN-
FIX” command is typed. 
Release  current  display  window  set  by  the  “FIX”, 
“GSET”, “FSET” or “SETF” commands. 
Zoom in at point (a,b) with window  l where a, b, and  l 
are numbers between 0 and 1.  The picture is assumed to 
lie in a unit square.
APPENDIX M 
UZG 
UZOU a b  l 
Z r z  l∆  
ZOUT r z  l∆ 
Cover currently displayed picture with a 10 by 10 square 
grid to aid in zooming with the unity zoom, “UZ”, com-
mand. 
Zoom out at point (a,b) with window  l where a, b, and  l 
are  numbers  between  0  and  1.    The  current  window  is 
scaled by the factor 1 ∆⁄ l.The picture is assumed to lie in a 
unit square. 
Zoom in at point (r,z) with window ∆l. 
∆
∆
Zoom out at point (r,z) with window  l.   The window is 
enlarged by the ratio of the current window and  l.  The 
cursor may be used to zoom out via the cursor command 
DZOU and entering two points with the cursor to define 
the  window.    The  ratio  of  the  current  window  with  the 
specified  window  determines  the  picture  size  reduction.  
An  alternative  cursor  command,  DZZO,  may  be  used 
and  only  needs  one  point  to  be  entered  at  the  location 
where the reduction (2×) is expected. 
Graphics Window Controls for x versus y plots 
The following commands apply to line plots, interface plots, etc. 
ASCL fa 
Scale all abscissa data by fa.  The default is fa = 1. 
ASET amin amax 
Set  minimum  and  maximum  values  on  abscissa  to  amin 
and  amax,  respectively.    If  amin = amax = 0.0  (default) 
LS-DYNA  determines  the  minimum  and  maximum  val-
ues. 
OSCL fo 
Scale all ordinate data by fo.  The default is fo = 1. 
OSET omin omax 
Set minimum and maximum values on ordinate to omin 
and  omax,  respectively.    If  omin = omax = 0.0  (default) 
LS-DYNA  determines  the  minimum  and  maximum  val-
ues. 
SMOOTH n 
Smooth a data curve by replacing each data point by the 
average of the 2n adjacent points.  The default is n = 0. 
Mesh Display Options 
ELPLT 
Plot element numbers on  mesh of material n.
FSOFF 
FSON 
G 
GO 
GS 
M n 
MNOFF 
MNON 
NDPLT 
O 
RPHA 
RPVA 
TN r z  l 
UG 
V 
VSF 
APPENDIX M 
Turn off the “FSON” command. 
Plot  only  free  surfaces  and  slideline  interfaces  with  “O” 
command.  (Must be used before “O” command.) 
View mesh. 
View  mesh  right  of  centerline  and  outline  left  of 
centerline. 
View mesh and solid fill elements to identify materials by 
color. 
Material n is to be rezoned. 
Do  not  plot  material  numbers  with  the  “O”,  “G”,  and 
“GO” commands (default). 
Plot  material  numbers  with  “O”,  “G”,  and  “GO” 
commands. 
Plot node numbers on mesh of material n. 
Plot outlines of all material. 
Reflect mesh, contour, fringe, etc., plots about horizontal 
axis.  Retyping “RPHA” turns this option off. 
Reflect  mesh,  contour,  fringe,  etc.,  plots  about  vertical 
axis.  Retyping “RPVA” turns this option off. 
Type  node  numbers  and  coordinates  of  all nodes  within 
window (r ± ∆l⁄2, z ± ∆l⁄2). 
Display undeformed mesh. 
Display  material  n  on  graphics  display.    See  command 
M. 
Display  material  n  on  graphics  display  and  solid  fill 
elements. 
Mesh Modifications 
BACKUP 
Restore  mesh  to  its  previous  state.    This  command 
undoes the result of the last command.
APPENDIX M 
BLEN s 
Smooth  option  where  s = 0  and  s = 1  correspond  to 
equipotential and isoparametric smoothing, respectively.  
By letting 0 ≤ s ≤ 1 a combined blending is obtained. 
CN m r z 
Node m has new coordinate (r,z). 
DEB n f1 l1 ...  fn ln 
Delete  n  element  blocks  consisting  of  element    numbers 
f1  to  l1,  f2  to  l2  ...    ,  and  fo  ln  inclusive.    These  elements 
will be inactive when the calculation resume. 
DE e1 e2 
Delete elements e1 to e2. 
DMB n m1 m2 ...  mn 
Delete  n  material  blocks  consisting  of  all  elements  with 
material  numbers  m1,  m2,...,  and  mn.    These  materials 
will be inactive when the calculations resume. 
DM n m1 m2 ...  mn 
Delete n materials including m1, m2,..., and mn. 
DZER k d incr nrow 
Delete element row where k is the kept element, d is the 
deleted  element,  incr  is  the  increment,  and  nrow  is  the 
number of elements in the row. 
DZLN number n1 n2 n3...nlast  Delete nodal row where number is the number of nodes 
in the row and n1, n2, ...  nlast are the ordered list of delet-
ed nodes. 
DZNR l j incr 
Delete nodal row where l is the first node in the row, j is 
the last node in the row, and incr is the increment. 
R 
S 
Restore original mesh. 
Smooth  mesh  of  material  n.    To  smooth  a  subset  of 
elements,  a  window  can  be  set  via  the  “GSET”,  “FSET”, 
OR  “SETF”  commands.    Only  the  elements  lying  within 
the window are smoothed. 
Boundary Modifications 
A 
B 
BD m n 
56-6 (APPENDIX M) 
Display  all  slidelines.    Slave  sides  are  plotted  as  dashed 
lines. 
Determine  boundary  nodes  and  sides  of  material  n  and 
display boundary with nodes and side numbers. 
Dekink  boundary  from  boundary  node  m  to  boundary
BDS s 
Dekink side s. 
DSL n l1 l2...ln 
Delete  n  slidelines  including  slideline  numbers  l1  l2..., 
and ln. 
APPENDIX M 
ER m n 
ERS s 
ES m n 
ESS s 
EZ m n 
EZS s 
MC n 
MD n 
MN n 
SC n 
SD n 
SLN m n 
SLNS n 
SN n 
Equal  space  in  r-direction  boundary  nodes  m  to  n 
(counterclockwise). 
Equal space in the r-direction boundary nodes on side s. 
Equal  space  along  boundary,  boundary  nodes  m  to  n 
(counterclockwise). 
Equal space along boundary, boundary nodes on side s. 
Equal  space  in  z-direction  boundary  nodes  m  to  n 
(counterclockwise). 
Equal space in the z-direction boundary nodes on side s. 
Check master nodes of slideline n and put any nodes that 
have  penetrated  through  the  slave  surface  back  on  the 
slave surface. 
Dekink  master  side  of  slideline  n.    After  using  this 
command, the SC or MC command is sometimes advisa-
ble. 
Display slideline n with master node numbers. 
Check slave nodes of slideline n and put any nodes that 
have  penetrated  through  the  master  surface  back  on  the 
master surface. 
Dekink  slave  side  of  slideline  n;  after  using  this 
command, the SC or MC command is sometimes advisa-
ble. 
Equal space boundary nodes between nodes m to n on a 
straight line connecting node m to n. 
Equal  space  boundary  nodes  along  side  n  on  a  straight 
line connecting the corner nodes. 
Display slideline n with slave node numbers.
APPENDIX M 
VS m n r 
VSS s r 
MAZE Line Definitions 
B 
LD n k l 
LDS n l 
M n 
Vary the spacing of boundary nodes m to n such that r is 
the  ratio  of  the  first  segment  length  to  the  last  segment 
length. 
Vary the spacing of boundary nodes on side s such that r 
is the ratio of the first segment length to the last segment 
length. 
Determine  boundary  nodes  and  sides  of  material  n  and 
display  boundary  with  nodes  and  side  numbers.    See 
command “M”. 
Line  definition  n  for  MAZE  includes  boundary  nodes  k 
to l 
Line definition n for MAZE consists of side number l. 
Material n is active for the boundary command B. 
Calculation Graphics Display Control Parameters 
MOLP 
Overlay the mesh on the contour, fringe, principal stress, 
and  principal  strain  plots.    Retyping  “MOLP”  turns  this 
option off. 
NLOC 
Do not plot letters on contour lines. 
NUMCON n 
Plot n contour levels.  The default is 9. 
PLOC 
RANGE r1 r2 
Plot  letters  on  contour  lines  to  identify  their  levels 
(default). 
Set the range of levels to be between r1 and r2 instead of 
in  the  range  chosen  automatically  by  LS-DYNA.    To  de-
activate this command, type RANGE 0 0. 
Calculation Graphics Display 
CONTOUR c n m1 m2...mn  Contour  component  number  c  on  n  materials  including 
materials m1, m2, ..., mn.  If n is zero, only the outline of 
material  m1  with  contours  is  plotted.    Component  num-
bers are given in Table 56-1.
FRINGE c n m1 m2...mn 
IFD n 
IFN l m 
IFP c m 
IFS m 
IFVA rc zc 
IFVS 
LINE c n m1 m2...mn 
NCOL n 
NLDF n n1 n2...n3 
NSDF m 
NSSDF l m 
APPENDIX M 
Fringe component number c on n materials including m1, 
m2,...,mn.    If  n  is  zero,  only  the  outline  of  material  m1 
with contours is plotted.  Component numbers are given 
in Table 56-1. 
Begin  definition  of  interface  n.    If  interface  n  has  been 
previously  defined,  this  command  has  the  effect  of  de-
stroying the old definition. 
Include boundary nodes l to m (counterclockwise) in the 
interface definition.  This command must follow the “B” 
command. 
Plot  component  c  of  interface  m.    Component  numbers 
are given in Table 56-2. 
Include  side  m  in  the  interface  definition.    Side  m  is 
defined for material n by the “B” command. 
Plot  the  angular  location  of  the  interface  based  on  the 
center point (rc,zc) along the abscissa.  Positive angles are 
measured counterclockwise from the y-axis. 
Plot  the  distance  along  the  interface  from  the  first 
interface node along the abscissa (default). 
Plot variation of component c along line defined with the 
“NLDF”,  “PLDF”,  “NSDF”,  or  the  “NSSDF”  commands 
given below.  In determining variation, consider n mate-
rials including material number m1, m2,...mn. 
Number of colors in fringe plots is n.  The default value 
for  n  is  6  which  includes  colors  magenta,  blue,  cyan, 
green,  yellow,  and  red.    An  alternative  value  for  n  is  5 
which eliminates the minimum value magenta. 
Define 
line  for  “LINE”  command  using  n  nodes 
including  node  numbers  n1,  n2,...nn.    This  line  moves 
with the nodes.  
Define  line  for  “LINE”  command  as  side  m.    Side  m  is 
defined for material n by the “B” command. 
Define  line  for  “LINE”  command  and  that  includes 
boundary nodes l to m (counterclockwise) in the interface
APPENDIX M 
definitions.    This  command  must  follow  the  “B”  com-
mand. 
PLDF n r1 z1...rn zn 
Define  line  for  “LINE”  command  using  n  coordinate 
pairs (r1,z1), (r2,z2), ...(rn,zn).  This line is fixed in space. 
PRIN c n m1 m2...mn 
PROFILE c n m1 m2...mn 
VECTOR c n m1 m2...mn 
Plot lines of principal stress and strain in the yz plane on 
n materials including materials m1, m2,...,mn.  If n is zero, 
only  the  outline  of  material  m1  is  plotted.    The  lines  are 
plotted in the principal stress and strain directions.  Per-
missible component numbers in Table M.1 include 0, 5, 6, 
100,  105,  106,...,etc.    Orthogonal  lines  of  both  maximum 
and  minimum  stress  are  plotted  if  components  0,  100, 
200, etc.  are specified. 
Plot component c versus element number for n materials 
including materials m1, m2,...,mn.  If n is  0/  then compo-
nent  c  is  plotted  for  all  elements.    Component  numbers 
are given in Table M.1. 
Make  a  vector  plot  of  component  c  on  n  materials 
including  materials  m1,  m2,...,mn.    If  n  is  zero,  only  the 
outline  of  material  m1  with  vectors  is  plotted.    Compo-
nent c may be set to “D” and “V” for vector plots of dis-
placement and velocity, respectively.
No.  Component  
No.  Component 
APPENDIX M 
y 
z 
hoop 
yz 
maximum principal 
minimum principal 
von Mises (Appendix A) 
21* 
ln (V⁄Vo) (volumetric strain) 
22* 
y-displacement 
z-displacement  
23* 
24*  maximum displacement  
y-velocity, y-heat flux 
25* 
z-velocity, y-heat flux 
26* 
27*  maximum velocity, maximum 
1 
2 
3 
4 
5  
6 
7 
8 
9 
28 
29 
30 
31 
32 
pressure or average strain 
maximum principal 
- minimum principal 
y minus hoop 
10 
11  maximum shear 
ij and kl normal 
12 
 
jk and li normal 
ij and kl shear 
jk and li shear 
y-deviatoric 
z-deviatoric 
hoop-deviatoric 
effective plastic strain 
temperature/internal energy  
density 
13 
14 
15 
16 
17 
18 
19* 
20* 
  41*-70*  element history variables 
71* 
r-peak acceleration 
76* 
heat flux 
ij normal 
jk normal 
kl normal 
li normal 
ij shear 
jk shear 
kl shear 
li shear 
relative volume V⁄Vo 
33 
34 
35 
36* 
37*  Vo⁄V-1 
38* 
39* 
bulk viscosity, Q 
P + Q 
40* 
density 
72* 
73* 
74* 
75* 
z-peak acceleration 
r-peak velocity 
z-peak velocity 
peak value of max.  in plane prin.  stress 
77* 
78* 
79* 
peak value of min in plane 
prin.  stress 
peak value of maximum hoop stress 
peak value of minimum hoopstress 
peak value of pressure 
Table 56-1.  Component numbers for element variables.  By adding 100, 200 300, 400, 
500  and  600  to  the  component  numbers  not  followed  by  an  asterisk,  component 
numbers  for  infinitesimal  strains,  lagrange  strains,  almansi  strains,  strain  rates, 
extensions,  and  residual  strain  are  obtained.    Maximum  and  minimum  principal 
stresses  and  strains  are  in  the  rz  plane.    The  corresponding  hoop  quantities  must  be 
examined  to  determine  the  overall  extremum.    ij,  jk,  etc.    normal  components  are 
normal to the ij, jk, etc side.  The peak value database must be flagged on Control Card 
4 in columns 6-10 or components 71-79 will not be available for plotting.
APPENDIX M 
  No. 
Component 
1 
2 
3 
4 
5 
6 
pressure 
shear stress  
normal force 
tangential force 
y-force 
z-force 
Table  56-2.    Component  numbers  for  interface  variables.    In  ax-
isymmetric geometries the force is per radian. 
Cursor Commands 
DBD a b 
DCN a b 
DCSN n a 
DCNM a b 
DER a b 
DES a b 
DEZ a b 
DTE a b 
DTN a b 
Use cursor to define points a and b on boundary.  Dekink 
boundary starting at a, moving counterclockwise, and end-
ing at b. 
Use  cursor  to  define  points  a  and  b.    The  node  closest  to 
point a will be moved to point b. 
Move nodal point n to point a defined by the cursor. 
Use cursor to define points a and b.  The node at point a is 
given the coordinate at point b. 
Use  cursor  to  define  points  a  and  b  on  boundary.    Equal 
space  nodes  in  r-direction  along  boundary  starting  at  a, 
moving counterclockwise, and ending at b. 
Use  cursor  to  define  points  a  and  b  on  boundary.    Equal 
space nodes along boundary starting at a, moving counter-
clockwise, and ending at b. 
Use  cursor  to  define  points  a  and  b  on  boundary.    Equal 
space  nodes  in  z-direction  along  boundary  starting  at  a, 
moving counterclockwise, and ending at b. 
Use  cursor  to  define  points  a  and  b  on  the  diagonal  of  a 
window.    The  element  numbers  and  coordinates  of  ele-
ments lying within the window are typed on the terminal. 
Use  cursor  to  define  points  a  and  b  on  the  diagonal  of  a 
window.    The  node  numbers  and  coordinates  of  nodal 
points lying within the window are typed on the terminal.
DTNC a 
DVS a b r 
DZ a b 
DZOUT a b 
DZZ a 
APPENDIX M 
Use cursor to define point a.  The nodal point number and 
nodal  coordinates of  the  node  lying  closest  to  point  a  will 
be printed. 
Use cursor to define points a and b on boundary.  Variable 
space nodes along boundary starting at a, moving counter-
wise, and ending at b.  The ratio of the first segment length 
to the last segment length is give by r (via terminal). 
Use  cursor  to  define  points  a  and  b  on  the  diagonal  of  a 
window for zooming. 
Enter two points with the cursor to define the window.  The 
ratio of the current window with the specified window de-
termines the picture size reduction. 
Use cursor to define point a and zoom in at this point.  The 
new window is .15 as  large as the previous window.  The 
zoom  factor  can  be  reset  by  the  crzf  command  for  the  .15 
default. 
DZZO a 
Zoom out at point a by enlarging the picture two times.
APPENDIX N 
APPENDIX N: 
Rigid-Body Dummies 
The  two  varieties  of  rigid  body  dummies  available  in  LS-DYNA  are  described  in  this 
appendix.  These are generated internally by including the appropriate *COMPONENT 
keyword.  A description of the GEBOD dummies begins on this page and the HYBRID 
III family on page N.7. 
GEBOD Dummies 
Rigid  body  dummies  can  be  generated  and  simulated  within  LS-DYNA  using  the 
keyword  *COMPONENT_GEBOD.    Physical  properties  of  these  dummies  draw  upon 
the  GEBOD  database  [Cheng  et  al.    1994]  which  represents  an  extensive  measurement 
program  conducted  by  Wright-Patterson  AFB  and  other  agencies.    The  differential 
equations  governing  motion  of  the  dummy  are  integrated  within  LS-DYNA  separate 
from  the  finite  element  model.    Interaction  between  the  dummy  and  finite  element 
structure is achieved using contact interfaces .  
neck
upper torso
middle torso
lower torso
head
right shoulder
right upper arm
right lower arm 
right hand
right 
upper 
right lower leg
right foot 
Figure 57-1.  50th percentile male dummy in the nominal position.
APPENDIX N 
The  dynamical  system  representing  a  dummy  is  comprised  of  fifteen  rigid  bodies 
(segments) and include: lower torso, middle torso, upper torso, neck, head, upper arms, 
forearms/hands, upper legs, lower legs, and feet.  Ellipsoids are used for visualization 
and  contact  purposes.      Shown  in  Figure  57-1  is  a  50th  percentile  male  dummy 
generated  using  the  keyword  command  *COMPONENT_GEBOD_MALE.    Note  that 
the  ellipsoids  representing  the  shoulders  are  considered  to  be  part  of  the  upper  torso 
segment and the hands are rigidly attached to the forearms. 
Each of the rigid segments which make up the dummy is connected to its neighbor with 
a joint which permits various relative motions of the segments.  Listed in the Table 57-2 
are the joints and their applicable degrees of freedom. 
Joint 
Name 
pelvis 
waist 
Degree(s) of Freedom 
1st 
2nd 
lateral flexion (x) 
forward flexion (y) 
lateral flexion (x) 
forward flexion (y) 
lower neck 
lateral flexion (x) 
forward flexion (y) 
upper neck 
lateral flexion (x) 
forward flexion (y) 
3rd 
torsion (z) 
torsion (z) 
torsion (z) 
torsion (z) 
shoulders 
abduction-adduction (x) 
internal-external rotation (z) 
flexion-extension (y) 
elbows 
flexion-extension (y) 
n/a 
n/a 
hips 
abduction-adduction (x) 
medial-lateral rotation (z) 
flexion-extension (y) 
knees 
flexion-extension (y) 
n/a 
n/a 
ankles 
inversion-eversion (x) 
dorsi-plantar flexion (y) 
medial-lateral rotation (z) 
Table 57-2.  Joints and associated degrees of freedom.  Local axes are in parentheses. 
Orientation of a segment is effected by performing successive right-handed rotations of 
that segment relative to its parent segment - each rotation corresponds to a joint degree 
of  freedom.    These  rotations  are  performed  about  the  local  segment  axes  and  the 
sequence  is  given  in  Table  57-2.    For  example,  the  left  upper  leg  is  connected  to  the 
lower torso by the left hip joint; the limb is first abducted relative to lower torso, it then 
undergoes  lateral  rotation,  followed  by  extension.    The  remainder  of  the  lower 
extremity (lower leg and foot) moves with the upper leg during this orientation process. 
By  default  all  joints  are  assigned  stiffnesses,  viscous  characteristics,  and  stop  angles 
which should give reasonable results in a crash simulation.  One or all default values of 
a  joint  may  be  altered  by  applying  the  *COMPONENT_GEBOD_JOINT_OPTION 
command  to  the  joint of  interest.    The  default  shape  of  the resistive  torque  load  curve 
used  by  all  joints  is  shown  in  Figure  57-6.    A  scale  factor  is  applied  to  this  curve  to 
obtain  the  proper  stiffness  relationship.    Listed  in  Table  57-3  are  the  default  values  of 
joint characteristics for dummies of all types and sizes.   These values are given in the
APPENDIX N 
English system of units; the appropriate units are used if a different system is specified 
in card 1 of *COMPONENT_GEBOD_OPTION. 
joint degrees 
of freedom 
load curve 
scale factor 
(in⋅lbf) 
damping 
coef. 
(in⋅lbf⋅s/rad)
low stop 
angle 
(degrees) 
high stop 
angle 
(degrees) 
neutral 
angle 
(degrees) 
pelvis - 1 
pelvis - 2  
pelvis - 3  
waist - 1 
waist - 2 
waist - 3 
lower neck - 1 
lower neck - 2 
lower neck - 3 
upper neck - 1 
upper neck - 2 
upper neck - 3 
l.  shoulder - 1 
r.  shoulder - 1 
shoulder - 2 
shoulder - 3 
elbow - 1 
l.  hip - 1 
r.  hip - 1 
hip - 2 
hip - 3 
knee - 1 
l.  ankle - 1 
l.  ankle - 1 
ankle - 2 
ankle - 3 
65000 
65000 
65000 
65000 
65000 
65000 
10000 
10000 
10000 
10000 
10000 
10000 
100 
100 
100 
100 
100 
10000 
10000 
10000 
10000 
100 
100 
100 
100 
100 
5.77 
5.77 
5.77 
5.77 
5.77 
5.77 
5.77 
5.77 
5.77 
5.77 
5.77 
5.77 
5.77 
5.77 
5.77 
5.77 
5.77 
5.77 
5.77 
5.77 
5.77 
5.77 
5.77 
5.77 
5.77 
5.77 
-20 
-20 
-5 
-20 
-20 
-35 
-25 
-25 
-35 
-25 
-25 
-35 
-30 
-175 
-65 
-175 
1 
-25 
-70 
-70 
-140 
-1 
-30 
-20 
-20 
-30 
20 
20 
5 
20 
20 
35 
25 
25 
35 
25 
25 
35 
175 
30 
65 
60 
-140 
70 
25 
70 
40 
120 
20 
30 
45 
30 
Table 57-3.  Default joint characteristics for all dummies. 
0 
0 
0 
0 
0 
0 
0 
0 
0 
0 
0 
0 
0 
0 
0 
0 
0 
0 
0 
0 
0 
0 
0 
0 
0
APPENDIX N 
torque
(-3.14,2.0)
(-0.5,0.1)
(0,0)
(0.5,-0.1)
rotation (radians)
(3.14,-2.0)
Figure 57-4  Characteristic torque curve shape used by all joints. 
The  dummy  depicted  in  Figure  57-1  appears  in  what  is  referred  to  as  its  "nominal" 
position.    In  this  position  the  dummy  is  standing  upright  facing  in  the  positive  x 
direction and the toe-to-head direction points in positive z.  Additionally, the dummy's 
hands are at the sides with palms facing inward and the centroid of the lower torso is 
positioned at the origin of the global coordinate system.  Each of the dummy's segments 
has a local coordinate system attached to it and in the nominal position all of the local 
axes are aligned with the global axes. 
When  performing  a  simulation  involving  a  *COMPONENT_GEBOD  dummy,  a 
positioning  file  named  "gebod.did"  must  reside  in  the  directory  with  the  LS-DYNA 
input  file;  here  the  extension  did  is  the  dummy  ID  number,  see  card  1  of  *COMPO-
NENT_GEBOD_OPTION.    The  contents  of  a  typical  positioning  file  is  shown  in Table 
57-5;  it  consists  of  40  lines  formatted  as  (59a1,e30.0).    All  of  the  angular  measures  are 
input as degrees, while the lower torso global positions depend on the choice of units in 
card 1 of *COMPONENT_GEBOD_OPTION.  Setting all of the values in this file to zero 
yields the so-called "nominal" position. 
Table 57-5.  Typical contents of a dummy positioning file. 
lower torso 
lower torso 
lower torso 
total body 
total body 
total body 
centroid global x position 
centroid global y position 
centroid global z position 
global x rotation 
global y rotation 
global z rotation 
0.0 
0.0 
0.0 
0.0 
-20.0 
180.0
APPENDIX N 
pelvis 
pelvis 
pelvis 
waist 
waist 
waist 
lower neck 
lower neck 
lower neck 
upper neck 
upper neck 
upper neck 
left shoulder 
left shoulder 
left shoulder 
right shoulder 
right shoulder 
right shoulder 
left elbow 
right elbow 
left hip 
left hip 
left hip 
right hip 
right hip 
right hip 
left knee 
right knee 
left ankle 
left ankle 
left ankle 
right ankle 
right ankle 
right ankle 
lateral  flexion 
forward  flexion 
torsion 
lateral  flexion 
forward  flexion 
torsion 
lateral  flexion 
forward  flexion 
torsion 
lateral  lexion 
forward  flexion 
torsion 
abduction-adduction 
internal-external rotation 
flexion-extension 
abduction-adduction 
internal-external rotation 
flexion-extension 
flexion-extension 
flexion-extension 
abduction-adduction 
medial-lateral rotation 
flexion-extension 
abduction-adduction 
medial-lateral rotation 
flexion-extension 
flexion-extension 
flexion-extension 
inversion-eversion 
dorsi-plantar flexion 
medial-lateral rotation 
inversion-eversion 
dorsi-plantar flexion 
medial-lateral rotation 
+ = tilt right 
+ = lean fwd 
+ = twist left 
+ = tilt right 
+ = lean fwd 
+ = twist left 
+ = tilt right 
+ = nod fwd 
+ = twist left 
+ = tilt right 
+ = nod fwd 
+ = twist left 
+ = abduction 
+ = external 
- = fwd raise 
- = abduction 
- = external 
- = fwd raise 
+ = extension 
+ = extension 
+ = abduction 
+ = lateral 
+ = extension 
- = abduction 
- = lateral 
+ = extension 
+ = flexion 
+ = flexion 
+ = eversion 
+ = plantar 
+ = lateral 
- = eversion 
+ = plantar 
- = lateral 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
30.0 
-10.0 
-40.0 
-30.0 
10.0 
-40.0 
-60.0 
-60.0 
0.0 
0.0 
-80.0 
0.0 
0.0 
-80.0 
50.0 
50.0 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
In Figure 57-6 the 50th percentile male dummy is shown in a seated position and some 
of its joints are labeled.  The file listed in Table 57-5 was used to put the dummy into the 
position  shown.    Note  that  the  dummy  was  first  brought  into  general  orientation  by 
setting nonzero values for two of the lower torso local rotations.  This is accomplished 
by  performing  right-handed  rotations  successively  about  local  axes  fixed  in  the  lower 
torso, the sequence of which follows:  the first about local x, next about local y, and the 
last about local z.   The dummy in Figure 57-6 was made to pitch  backward by setting
APPENDIX N 
"total  body  global  y  rotation"  equal  to  -20.    Setting  the  "total  body  global  z  rotation" 
equal  to  180  caused  the  dummy  to  rotate  about  the  global  z-axis  and  face  in  the  -x 
direction. 
upper neck
lower neck
left elbow
left shoulder
waist
pelvis
left hip 
left knee
left ankle
Figure 57-6.  Dummy seated using the file listed in Table 57-5.
HYBRID III Dummies 
A listing of applicable joint degrees of freedom of the Hybrid III dummy is given below. 
APPENDIX N 
Joint 
Name 
lumbar 
lower neck 
upper neck 
1st 
flexion (y) 
flexion (y) 
flexion (y) 
Degree(s) of Freedom 
2nd 
torsion (z) 
torsion (z) 
torsion (z) 
shoulders 
flexion-extension (y) 
abduction-adduction (x) 
elbows 
flexion-extension (y) 
wrists 
flexion-extension (x) 
n/a 
n/a 
3rd 
n/a 
n/a 
n/a 
hips  abduction-adduction (x) medial-lateral rotation (z) 
flexion-extension (y) 
knees 
flexion-extension (y) 
n/a 
n/a 
ankles 
inversion-eversion (x)  medial-lateral rotation (z) 
dorsi-plantar flexion (y) 
sternum 
translation (x) 
rotation (y) 
rotation (z) 
knee sliders 
translation (z) 
Table 57-7.  Joints and associated degrees of freedom.  Local axes are in parentheses. 
Joint  springs  of  the  *COMPONENT_HYBRIDIII  dummies  are  formulated  in  the 
following manner. 
𝑇 = 𝑎lo(𝑞 − 𝑞lo) + 𝑏lo(𝑞 − 𝑞lo)3,
𝑇 = 𝑎hi(𝑞 − 𝑞hi) + 𝑏hi(𝑞 − 𝑞hi)3,
𝑇 = 0,
𝑞 ≤ 𝑞lo
𝑞 ≥ 𝑞hi
𝑞lo < 𝑞 < 𝑞hi
Where, 
T is the joint torque 
q is the joint generalized coordinate 
alo and blo are the linear and cubic coefficients, respectively, for the low regime 
ahi and bhi are the linear and cubic coefficients, respectively, for the high regime 
qlo and qhi are the activation values for the low and high regimes, respectively
APPENDIX O 
APPENDIX O:  LS-DYNA 
MPP User Guide 
This is a short user’s guide for the MPP version of LS-DYNA.  For a general guide to the 
capabilities of LS-DYNA and a detailed description of the input, consult the LS-DYNA 
User's  Manual.    If  you  have  questions  about  this  guide,  find  errors  or  omissions  in  it, 
please email manual@lstc.com. 
SUPPORTED FEATURES 
The only input formats currently supported are 920 and later, including keyword input.  
Models  in  any  of  the  older  formats  will  need  to  be  converted  to  one  of  these  input 
formats  before  they  can  be  run  with  the  current  version  of  LS-DYNA  for  massively 
parallel processors, mpp. 
The  large  majority  of  LS-DYNA  options  are  available  on  MPP  computers.    Those  that 
are not supported are being systematically added.  Unless otherwise noted here, all the 
options of LS-DYNA version 93x are supported by MPP/LS-DYNA. 
Here is the list of unsupported features: 
*BOUNDARY_THERMAL_WELD 
*BOUNDARY_USA_SURFACE 
*CONTACT_1D 
*DATABASE_AVS 
*DATABASE_MOVIE 
*DATABASE_MPGS 
*LOAD_SUPERPLASTIC_OPTION 
*USER 
*TERMINATION_NODE 
CONTACT INTERFACES 
MPP/LS-DYNA  uses  a  completely  redesigned,  highly  parallel  contact  algorithm.    The 
contact options currently unsupported include:
Because these options are all supported via the new, parallel contact algorithms, slight 
differences  in  results  may  be  observed  as  compared  to  the  serial  and  SMP  versions  of 
LS-DYNA.    Work  has  been  done  to  minimize  these  differences,  but  they  may  still  be 
evident in some models. 
For  each  of  the  supported  CONTACT_control  cards,  there  is  an  optional  string_MPP 
which  can  be  appended  to  the  end.    Adding  these  characters  triggers  the  reading  of  a 
new  control  card  immediately  following  (but  after  the  TITLE  card,  if  any).    See  the 
section on *CONTACT for details of the parameters and their meanings. 
OUTPUT FILES AND POST-PROCESSING 
For performance reasons, many of the ASCII output files normally created by LS-DYNA 
have  been  combined  into  a  new  binary  format  used  by  MPP/LS-DYNA.    There  is  a 
post-processing program l2a, which reads this binary database of files and produces as 
output  the  corresponding  ASCII  files.    The  new  binary  files  will  be  created  in  the 
directory specified as the global directory in the pfile .  The files (up to 
one  per  processor)  are  named  binoutnnnn,  where  nnnn  is  replaced  by  the  four-digit 
processor number.  To convert these files to ASCII simply feed them to the l2a program 
like this: 
l2a binout* 
LS-PREPOST is able to read the binout files directly, so conversion is not required, it is 
provided for backward compatibility. 
The supported ASCII files are: 
*DATABASE_SECFORC 
*DATABASE_RWFORC 
*DATABASE_NODOUT 
*DATABASE_NODOUTHF 
*DATABASE_ELOUT 
*DATABASE_GLSTAT 
*DATABASE_DEFORC 
*DATABASE_MATSUM 
*DATABASE_NCFORC
*DATABASE_SPCFORC 
*DATABASE_SWFORC 
*DATABASE_DEFGEO 
*DATABASE_ABSTAT 
*DATABASE_NODOFR 
*DATABASE_BNDOUT 
*DATABASE_GCEOUT 
*DATABASE_RBDOUT 
*DATABASE_SLEOUT 
*DATABASE_JNTFORC 
*DATABASE_SBTOUT 
*DATABASE_SPHOUT 
*DATABASE_TPRINT 
Some  of  the  normal  LS-DYNA  files  will  have  corresponding  collections  of  files 
produced by MPP/LS-DYNA, with one per processor.  These include the d3dump files 
(new  names  =  d3dump.nnnn),  the  messag  files  (now  mesnnnn)  and  others.    Most  of 
these will be found in the local directory specified in the pfile. 
The  format  of  the  d3plot  file  has  not  been  changed.    It  will  be  created  in  the  global 
directory, and can be directly handled with your current graphics post-processor. 
PARALLEL SPECIFIC OPTIONS 
There are a few new command line options that are specific to the MPP version of LS-
DYNA. 
In the serial and SMP versions of LS-DYNA, the amount of memory required to run the 
problem can be specified on the command line by adding  “memory=XXX”, where XXX 
is the number of words of memory to be allocated.  For the MPP code, this will result in 
each  processor  allocating  XXX  words  of  memory.    If  pre-decomposition  has  not  been 
performed,  one  processor  must  perform  the  decomposition  of  the  problem.    This  can 
require  substantially  more  memory  than  will  be  required  once  execution  has  started.  
For  this  reason,  there  is  a  second  memory  command  line  option,  “memory2=YYY”.    If
APPENDIX O 
used  together  with  adding    “memory=XXX”,  the  decomposing  processor  will  allocate 
XXX words of memory, and all other processors will allocate YYY words of memory. 
For  example,  in  order  to  run  a  250,000  element  crash  problem  on  4  processors,  you 
might  need  memory=80m  and  memory2=20m.    To  run  the  same  problem  on  16 
processors,  you  still  need  memory=80m,  but  can  set  memory2=6m.    The  value  for 
memory2 drops nearly linearly with the number of processors used to run the program, 
which works well for shared-memory systems. 
Execution of the implicit solver in MPP requires a balance of memory across all of the 
processes.    The  user  should  not  use  memory2=  specification  for  runs  involving  the 
implicit  solver.    If  the  model  decomposition  cannot  be  performed  for  the  given 
memory= specification, one can try a pre-decomposition but the user would be advised 
to  use  a  compute  cluster  with  more  real  memory.    It  is  suggested  that  the  memory= 
specification  be  such  to  use  no  more  than  75%  of  the  real  memory  available  to  that 
process.  On a compute cluster with each compute node having 48 Gbytes of memory 
and  using  8  MPI  processes,  there  is  only  6  Gbytes  of  real  memory  per  process.  
Converting  to  8  byte  words  and  using  only  the  suggested  75%  would  have 
memory=560M as the maximum specification. 
The full deck restart capability is supported by the MPP version of LS-DYNA, but in a 
manner slightly different than the SMP code.  Each time a restart dump file is written, a 
separate restart file is also written with the base name D3FULL.  For example, when the 
third  restart  file  d3dump03  is  written  (one  for  each  processor,  d3dump03.0000, 
d3dump03.0001,  etc),  there  is  also  a  single  file  written  named  d3full03.    This  file  is 
required in order to do a full deck restart and the d3dump files are not used in this case 
by the MPP code.  In order to perform a full deck restart with the MPP code, you first 
must prepare a full deck restart input file as for the serial/SMP version.  Then, instead 
of  giving  the  command  line  option  r=d3dump03  you  would  use  the  special  option 
n=d3full03.  The presence of this command line option tells the MPP code that this is a 
restart, not a new problem, and that the file d3full03 contains the  geometry and stress 
data carried over from the previous run. 
PFILE 
There is a new command line option: p = pfile.  pfile contains MPP specific parameters 
that  affect  the  execution  of  the  program.    The  file  is  split  into  sections,  with  several 
options  in  each  section.    Currently,  these  sections:  directory,  decomposition,  contact, 
and general are available.  First, here is a sample pfile: 
directory { 
global rundir 
local /tmp/rundir 
} 
contact {
APPENDIX O 
inititer 3 
} 
The  file  is  case  insensitive  and  free  format  input.    The  sections  and  options  currently 
supported are: 
directory:  Holds directory specific options 
transfer_files 
If  this  option  is  given,  then  processor  0 will  write  all  output  and  restart  files  to 
the global directory , and scratch files to the local directory.  
All other processors will write all data to their local directory.  At normal termi-
nation, all restart and output files will be copied from the processor specific local 
directories to the global directory.  Also, if this is a restart from a dump file, the 
dump files will be distributed to the processors from the global directory.  With 
this option enabled, there is no need for the processors to have shared access to a 
single  disk  for  output  –  all  files  will  be  transferred  as  needed  to  and  from  the 
global directory. 
Default = disabled. 
global path 
Path to a directory where program output should be written.  If transfer_files is 
not given, this directory needs to be accessible to all processors – otherwise it is 
only accessed by processor 0.  This directory will be created if necessary. 
Default = current working directory 
global_message_files 
If this option appears, the message files are written in the global directory rather 
than the local directory 
Default = disabled (message files go in the local directory) 
local path 
Path to a processor specific local directory for scratch files.  This directory will be 
created  if  necessary.    This  should  be  a  local  disk  on  each  processor,  for  perfor-
mance reasons. 
Default = global path 
rmlocal 
If this option is given and transfer_files is active, the program attempts to clean 
up the local directories on each processor.  In particular, it deletes files that are 
successfully  transferred  back  to  the  global  directory,  and  removes  the  local 
directory if it was created.  It will not delete any files if there is a failure during 
file copying, nor will it delete directories it did not create. 
Default = disabled 
repository path
APPENDIX O 
Path to a safe directory accessible from processor 0.  This directory will be creat-
ed  if  necessary.    This  is  intended  to  be  used  as  a  safekeeping/backup  of  files 
during execution and should only be used if transfer_files is also given.  If this 
directory is specified then the following actions occur: 
•  At program start up, any required files (d3dump, binout, etc) that can-
not  be  located  in  the  global  directory  are  looked  for  in  the  repository 
for copying to the local processor directories. 
•  Important output files (d3dump, runrsf, d3plot, binout and others) are 
synchronized  to  the  repository  regularly.    That  is,  every  time  one  of 
these files is updated on the node local or the global directories, a syn-
chronized copy is updated in the repository. 
The intention is that the repository be on a redundant disk, such as NAS, to allow 
restarting  the  problem  if  a  hardware  failure  should  occur  on  the  machine  run-
ning the problem.  It must be noted that some performance penalty must be paid 
for  the  extra  communication  and  I/O.    Effort  has  been  made  to  minimize  this 
overhead, but this option is not recommended for general use. 
Default = unspecified 
decomposition:  Holds decomposition specific options 
file filename 
The name of the file that holds the decomposition information.  This file will be 
created in the current working directory if it does not exist.  If this option is not 
specified, MPP/LS-DYNA will perform the decomposition. 
Default = None 
numproc n 
The problem will be decomposed for n processors.  If n > 1 and you are running 
on  1  processor,  or  if  the  number  of  processors  you  are  running  on  does  not 
evenly  divide  n,  then  execution  terminates  immediately  after  decomposition.  
Otherwise,  the  decomposition  file  is  written  and  execution  continues.    For  a 
decomposition only run, both numproc and file should be specified. 
Default = the number of processors you are running on. 
method name 
Currently,  there  are  two  decomposition  methods  supported,  namely  rcb  and 
greedy.  Method rcb is Recursive Coordinate Bisection.  Method greedy is a simple 
neighborhood  expansion  algorithm.    The  impact  on  overall  runtime  is  problem 
dependent, but rcb generally gives the best performance. 
Default = rcb 
region rx ry rz sx sy sz c2r s2r 3vec mat 
See the section below on Special Decompositions for details about these decom-
position options.
APPENDIX O 
show 
If this option appears in the decomposition section, the d3plot file is doctored so 
that  the  decomposition  can  be  viewed  with  the  post  processor.    Displaying 
material 1 will show that portion of the problem assigned to processor 0, and so 
on.    The  problem  will  not  actually  be  run,  but  the  code  will  terminate  once  the 
initial d3plot state has been written. 
rcblog filename 
This  option  is  ignored  unless  the  decomposition  method  is  RCB.    A  record  is 
written  to  the  indicated  file  recording  the  steps  taken  during  decomposition.  
This is an ascii file giving each decomposition region  and the location of each subdivision for that region.  Except for 
the addition of this decomposition information, the file is otherwise equivalent to 
the current pfile.  Thus it can be used directly as the pfile for a subsequent prob-
lem, which will result in a decomposition as similar as possible between the two 
runs.  For example, suppose a simulation is run twice, but the second time with a 
slightly  different  mesh.    Because  of  the  different  meshes  the  problems  will  be 
distributed  differently  between  the  processors,  resulting  in  slightly  different 
answers due to roundoff errors.  If an rcblog is used, then the resulting decompo-
sitions would be as similar as possible. 
vspeed 
If this option is specified a brief measurement is taken of the performance of each 
processor by timing a short floating point calculation.  The resulting information 
is  used  during  the  decomposition  to  distribute  the  problem  according  to  the 
relative  speed  of  the  processors.    This  might  be  of  some  use  if  the  cluster  has 
machines of significantly different speed. 
automatic 
If this option is given, an attempt is made to automatically determine a reasona-
ble decomposition, primarily based on the initial velocity of nodes in the model.  
Use of the show option is recommended to verify a reasonable decomposition. 
aledist 
Distribute ALE elements to all processors.   
dcmem n 
It may be in some cases that the memory requirements during the first phase of 
decomposition  are  too  high.    If  that  is  found  to  be  the  case  (if  you  get  out  of 
memory  errors  during  decomposition  phase  1),  then  this  may  provide  a  work 
around.  Specifying a value n here will cause some routines to process the model 
in  blocks  of  n  items,  when  normal  processing  would  read  the  whole  set  (of 
nodes, elements, whatever) all at once.  This will reduce memory requirements at 
the  cost  of  greater  communication  overhead.    Most  users  will  not  need  this 
option.  Values in the range of 10,000 to 50,000 would be reasonable.
APPENDIX O 
dunreflc 
Time  dependent  load  curves  are  usually  applied  to  the  following  boundary  or 
loading conditions on each node.  By default, those curves are copied to all MPP 
subdomain without checking for the presence of that node in the domain or not.  
The  curves  are  evaluated  every  cycle  and  may  consume  substantial  CPU  time.  
This command will remove curves which are  not referenced in the MPP subdo-
main for the following keywords. 
*BOUNDARY_PRESCRIBED_MOTION_NODE 
*LOAD_NODE 
*LOAD_SHELL_ELEMENT 
*LOAD_THERMAL_VARIABLE_NODE 
timing_start n 
Begin  timing  of  element  calculations  on  cycle  n.    The  appearance  of  this  option 
will  trigger  the  generation  of  a  file  named  DECOMP_TIMINGS.OUT  during 
normal  termination.    This  file  will  contain  information  about  the  actual  time 
spent doing element calculations, broken down by part. 
timing_end n 
End  timing  of  element  calculations  on  cycle  n.    A  reasonable  value  is  probably 
timing_start + 50 or 100. 
timing_file filename 
The file filename is assumed to be the output file DECOMP_TIMINGS.OUT from 
a  previous  run  of  this  or  a  similar  model.    The  computational  cost  of  each  part 
that appears in this file is then used during the decomposition instead of the built 
in internal value for that part.  Matching is based strictly on the user part ID.  The 
first two lines of the file are skipped, and only the first two entries on each of the 
remaining lines are relevant (the part ID and the cost per element). 
contact: 
This section has been  largely replaced by the_MPP option on the normal contact card.  
The only remaining useful option here is: 
alebkt n 
Sets the bucket sort frequency for FSI (fluid structure interaction) to once every n 
cycles. 
default = 50 
general:  Holds general options
APPENDIX O 
lstc_reduce 
If  this  option  appears,  LSTC’s  own  reduce  routine  is  used  to  get  consistent 
summation  of  floating  point  data  among  processors.    See  also,  *CONTROL_MPP_-
IO_LSTC_REDUCE which has the same effect.. 
nodump 
If this option appears, all restart dump file writing will be suppressed: d3dump, 
runrsf, and d3full files will not be written 
nofull 
If this option appears, writing of d3full (full deck restart) files will be suppressed. 
nod3dump 
If this option appears, writing of d3dump and runrsf files will be suppressed. 
runrsfonly 
If this option appears, writing of d3dump files will not occur – runrsf files will be 
witten instead.  Any time a d3dump OR runrsf file would normally be written, a 
runrsf file will be written. 
nofail 
If this option appears, the check for failed elements in the contact routines will be 
skipped.    This  can  improve  efficiency  if  you  do  not  have  element  failure  in  the 
model. 
swapbytes 
If  this  option  appears,  the  d3plot  and  interface  component  analysis  files  are 
written in swapped byte ordering. 
nobeamout 
Generally,  whenever  a  beam,  shell,  or  solid  element  fails,  and  element  failure 
report is written to the d3hsp and message files.  This can generate a lot of out-
put.  If this option appears, the element failure report is suppressed. 
Special Decompositions: 
These  options  appear  in  the  “decomposition”  section  of  the  pfile  and  are  only  valid  if 
the decomposition method is rcb.  The rcb decomposition method works by recursively 
dividing  the  model  in  half,  each  time  slicing  the  current  piece  of  the  model 
perpendicularly to one of the three coordinate axes.  It chooses the axis along which the 
current piece of the model is longest.  The result is that it tends to generate cube shaped 
domains  aligned  along  the  coordinate  axes.    This  is  inherent  in  the  algorithm,  but  is 
often not the behavior desired.
APPENDIX O 
This  situation  is  addressed  by  providing  a  set  of  coordinate  transformation  functions 
which  are  applied  to  the  model  before  it  is  decomposed.    The  resulting  deformed 
geometry is then passed to the decomposition algorithm, and the resulting domains are 
mapped  back  to  the  undeformed  model.    As  a  simple  example,  suppose  you  wanted 
rectangular  domains  aligned  along  a  line  in  the  xy  plane,  30  degrees  from  the  x  axis, 
and twice as long along this line as in the other two dimensions.  If you applied these 
transformations: 
sx 0.5 
rz -30 
then you would achieve the desired effect. 
Furthermore, it may be desirable for different portions of the model to be decomposed 
differently.    It  is  now  possible  to  specify  different  regions  of  the  model  to  be 
decomposed  with  different  transformations. 
  The  general  form  for  a  special 
decomposition would look like this: 
decomposition { 
region { <region specifiers> <transformation> <grouping> } 
region { <region specifiers> <transformation> <grouping> } 
<transformation> 
} 
Where the region specifiers are logical combinations of box, sphere, clinder, parts, and 
silist. 
The  transformation  is  a  series  of  sx,  sy,  sz,  rx,  ry,  rz,  c2r,  s2r,  3vec,  and  mat.    The 
grouping is either lumped or empty.  The portion of the model falling in the first region 
will be decomposed according to the given transformation.  Any remaining part of the 
model  in  the  second  region  will  then  be  treated,  and  finally  anything  left  over  will  be 
decomposed  according  to  the  final  transformation.    Any  number  of  regions  may  be 
given, including 0.  Any number of transformations may be specified.  They are applied 
to the region in the order given. 
The region specifiers are: 
box xmin xmax ymin ymax zmin zmax 
A box with the given extents. 
sphere xc yc zc r 
The sphere centered at (xc,yc,zc) and having radius r.  If r is negative it is treated as 
infinite. 
cylinder xc yc zc ax ay az r d 
A cylinder with center at (xc,yc,zc) and radius r, extending out in the direction of 
(ax,ay,az) for a distance of d.  If d is 0, the cylinder is infinte in both directions.
APPENDIX O 
parts n1 n2 n3 n4…. 
All parts whose user id matches one of the given values are included in the region.  
Any number of values may be given. 
partsets n1 n2 n3 n4…. 
All  partsets  whose  user  id  matches  one  of  the  given  values  will  have  all  of  their 
parts included in the region.  Any number of values may be given. 
silist n1 n2 n3 n4…. 
All  elements  involved  in  a  contact  interface  whose  user  id  matches  one  of  the 
given values are included in the region. 
The transformations available are: 
local 
This  is  only  useful  in  conjunction  with  the  *CONTROL_MPP_PFILE  keyword 
option,  when  used  inside  a  file  included  via  *INCLUDE_TRANSFORM.    At  this 
point  in  the  region  processing,  a  transformation  is  inserted  to  invert the transfor-
mation used by *INCLUDE_TRANSFORM.  The effect is that if this option appears 
before  any  other  transformation  options,  all  those  options  (and  the  subsequent 
decomposition)  are  performed  in  the  coordinate  system  of  the  include  file  itself, 
not the global coordinate system.. 
sx t 
scale the current x coordinates by t. 
sy t 
scale the current y coordinates by t. 
sz t 
scale the current z coordinates by t. 
rx t 
rotate around the current x axis by t degrees. 
ry t 
rotate around the current y axis by t degrees. 
rz t 
rotate around the current z axis by t degrees. 
txyz x y z 
translate by (x,y,z). 
mat m11 m12 m13 m21 m22 m23 m31 m32 m33 
transform the coordinates by matrix multiplication:
APPENDIX O 
Transformed Coordinates =
𝑥′
⎤ =
⎡
𝑦′
⎥
⎢
𝑧′⎦
⎣
𝑚11 𝑚12 𝑚13
⎥⎤ [
⎢⎡
𝑚21 𝑚22 𝑚23
𝑚31 𝑚32 𝑚33⎦
⎣
] 
3vec v11 v12 v13 v21 v22 v23 v31 v32 v33 
Transform the coordinates by the inverse of the transpose matrix: 
𝑣11
⎢⎡
𝑣12
𝑣13
⎣
𝑣31
⎥⎤
𝑣32
𝑣33⎦
𝑣21
𝑣22
𝑣23
𝑥′
⎤ 
⎡
𝑦′
⎥
⎢
𝑧′⎦
⎣
] =
[
= VT × transformed coordinates 
This appears complicated, but in practice is very intuitive: instead of decomposing 
into cubes aligned along the coordinate axes, rcb will decompose into parallelipi-
peds  whose  edges  are  aligned  with  the  three  vectors  (v11,  v12,  v13),  (v21,  v22, 
v23),  and  (v31,  v32,  v33).        Furthermore,  the  relative  lengths  of  the  edges  of  the 
decomposition domains will correspond to the relative lengths of these vectors. 
C2R x0 y0 z0 vx1 vy1 vz1 vx2 vy2 vz2 
The  part  is  converted  into  a  cylindrical  coordinate  system  with  origin  at  (x0,  y0, 
z0),  cylinder  axis  (vx1,  vy1,  vz1)  and  theta = 0  along  the  vector  (vx2,  vy2,  vz2).  
You  can  think  of  this  as  tearing  the  model  along  the  (vx2,  vy2,  vz2)  vector  and 
unwrapping it around the (vx1, vy1, vz1) axis.  The effect is to create decomposi-
tion  domains  that  are  “cubes”  in  cylindrical  coordinates:  they  are  portions  of 
cylindrical shells.  The actual transformation is: 
new(𝑥, 𝑦, 𝑧) = cylindrical coordinates(𝑟, 𝜃, 𝑧) 
Knowing  the  order  of  the  coordinates  is  important  if  combining  transformations, 
as in the example below. 
S2R x0 y0 z0 vx1 vy1 vz1 vx2 vy2 vz2 
Just  like  the  above,  but  for  spherical  coordinates.    The  (vx1,vy1,vz1)  vector  is  the 
phi = 0 axis. 
new(𝑥, 𝑦, 𝑧) = spherical coordinates(𝜌, 𝜃, 𝜙) 
The grouping qualifier is: 
lumped 
Group all elements in the region on a single processor.  If this qualifier is not given, 
the elements in the region are distributed across all processors. 
Examples: 
rz 45 
will generate domains rotated -45 degrees around the z axis.
APPENDIX O 
C2R 0 0 0 0 0 1 1 0 0 
will  generate  cylindrical  shells  of  domains.    They  will  have  their  axis  along  the 
vector (0,0,1), and will start at the vector (1,0,0) Note that the part will be cut at 
(1,0,0), so no domains will cross this boundary.  If there is a natural boundary or 
opening  in  your  part, the  “theta = 0” vector should  point  through this  opening.  
Note also that if the part is, say, a cylinder 100 units tall and 50 units in radius, 
after the C2R transformation the part will fit inside the  box x=[0,50], y=[0, 2PI), 
z=[0,100].    In  particular,  the  new  y  coordinates  (theta)  will  be  very  small  com-
pared to the other coordinate directions.  It is therefore likely that every decom-
position domain will extend through the complete transformed y direction.  This 
means that each domain will be a shell completely around the original cylinder.  
If  you  want  to  split  the  domains  along  radial  lines,  try  this  pair  of  transfor-
mations: 
C2R 0 0 0 0 0 1 1 0 0 
SY 5000 
This will do the above C2R, but then scale y by 5000.  This will result in the part 
appearing  to  be  about  30,000  long  in  the  y  direction  --  long  enough  that  every 
decomposition  domain  will  divide  the  part  in  this  (transformed)  y  direction.  
The result will be decomposition domains that are radial “wedges” in the origi-
nal part. 
General  combinations  of  transformations  can  be  specified,  and  they  are  applied  in 
order: 
SX 5 SY .2 RZ 30 
will scale x, then y, then rotate. 
A more general decomposition might look like: 
decomposition { rx 45 sz 10 
region { parts 1 2 3 4 5 and sphere 0 0 0 200 lumped } 
region { box 0 100 –1.e+8 1.e+8 0 500 or sphere 100 0 200 200 rx 20 } 
} 
This would take elements that have user ID  1, 2, 3, 4, or 5 for their part, AND that lie in 
the sphere of radius 200 centered at (0,0,0), and place them all on one processor. 
Then,  any  remaining  elements  that  lie  in  the  given  box  OR  the  sphere  of  radius  200 
centered  at  (100,0,200)  would  be  rotated  20  degress  in  x  then  decomposed  across  all 
processors.  Finally, anything remaining would be rotated 45 degrees in x, scaled 10 in 
z, and distributed to all processors.  In general, region qualifiers can be combined using 
the logical operations and, or, and not.  Grouping using parentheses is also supported.
APPENDIX O 
EXECUTION OF MPP/LS-DYNA 
MPP/LS-DYNA  runs  under  a  parallel  environment  which  provided  by  the  hardware 
vendor.  The execution of the program therefore varies from machine to machine.  On 
some platforms, command line parameters can be passed directly on the command line.  
For  others,  the  use  of  the  names  file  is  required.    The  names  file  is  supported  on  all 
systems. 
The serial/SMP code supports the use of the SIGINT signal (usually Ctrl-C) to interrupt 
the execution and prompt for user input, generally referred to as “sense switches.”  The 
MPP  code  also  supports  this  capability.    However,  on  many  systems  a  shell  script  or 
front end program (generally “mpirun”) is required to start MPI applications.  Pressing 
Ctrl-C  on  some  systems  will  kill  this  process,  and  thus  kill  the  running  MPP-DYNA 
executable.    As  a  workaround,  when  the  MPP  code  begins  execution  it  creates  a  file 
“bg_switch”  in  the  current  working  directory.    This  file  contains  the  following  single 
line: 
rsh <machine name> kill -INT <PID> 
where < machine name > is the hostname of the machine on which the root MPP-DYNA 
process  is  running,  and  <PID>  is  its  process  id.    (on  HP  systems,  “rsh”  is  replaced  by 
“remsh”).  Thus, simply executing this file will send the appropriate signal. 
Here is a simple table to show how to run the program on various platforms.  Of course, 
scripts are often written to mask these differences. 
Platform 
Execution Command 
DEC Alpha 
dmpirun –np n mpp-dyna 
Fujitsu 
Hitachi 
HP 
IBM 
NEC 
SGI 
Sun 
jobexec –vp n –mem m mpp-dyna 
mpirun –np n mpp-dyna 
mpp-dyna –np n 
#!/bin./ksh 
export MP_PROC=n 
export MP_LABELIO=no 
export MP_EUILIB=us 
export MPI_EUIDEVICE=css0 
poe mpp-dyna 
mpirun –np n mpp-dyna 
mpirun –np n mpp-dyna 
tmrun –np n mpp-dyna
Where  n  is  the  number  of  processors,  mpp-dyna  is  the  name  of  the  MPP/LS-DYNA 
executable, and m is the MB of real memory.
APPENDIX O
APPENDIX P 
APPENDIX P:  Implicit Solver 
INTRODUCTION 
The  terms  implicit  and  explicit  refer  to  time  integration  algorithms.    In  the  explicit 
approach,  internal  and  external  forces  are  summed  at  each  node  point,  and  a  nodal 
acceleration  is  computed  by  dividing  by  nodal  mass.    The  solution  is  advanced  by 
integrating  this  acceleration  in  time.    The  maximum  time  step  size  is  limited  by  the 
Courant  condition,  producing  an  algorithm  which  typically  requires  many  relatively 
inexpensive time steps. 
While explicit analysis is well suited to dynamic simulations such as impact and crash, 
it can become prohibitively expensive to conduct long duration or static analyses.  Static 
problems  such  as  sheet  metal  springback  after  forming  are  one  application  area  for 
implicit  methods.    In  the  implicit  method,  a  global  stiffness  matrix  is  computed, 
inverted,  and  applied  to  the  nodal  out-of-balance  force  to  obtain  a  displacement 
increment.  The advantage of this approach is that time step size may be selected by the 
user.    The  disadvantage  is  the  large  numerical  effort  required  to  form,  store,  and 
factorize  the  stiffness  matrix.    Implicit  simulations  therefore  typically  involve  a 
relatively small number of expensive time steps. 
In  a  dynamic  implicit  simulation  these  steps  are  termed  time  steps,  and  in  a  static 
simulation they are load steps.  Multiple steps are used to divide the nonlinear behavior 
into manageable pieces, to obtain results at intermediate stages during the simulation, 
or perhaps to resolve a particular frequency of motion in dynamic simulations.  In each 
step, an equilibrium geometry is sought which balances dynamic, internal and external 
forces in the model.  The nonlinear equation solver performs an iterative search using one 
of  several  Newton  based  methods.    Convergence  of  this  iterative  process  is  obtained 
when  norms  of  displacement  and/or  energy  fall  below  user-prescribed  tolerances.  
Within each implicit iteration there is a line search performed for enhancing robustness 
of the procedure. 
The  implicit  analysis  capability  was  first  released  in  Version  950.    Initially  targeted  at 
metal forming springback simulation, this new capability allowed static stress analysis.  
Version  970  added  many  additional  implicit  features,  including  new  element 
formulations for linear and modal analysis.  A milestone in implicit was the advent of 
Version 971 in which implicit analysis was carried over to MPP and thus allowed much 
larger  problems  to  be  solved,  and  from  there  it  has  evolved  extensively  to  presently 
contend well among competitive softwares.  Still, it can be a gruesome task to set up an 
implicit  input  problem  that  runs  all  the  way  to  completion  with  acceptable  results, 
especially when contacts are involved.  The purpose of this text is to explain keywords 
of interest and suggest values of important parameters in order to give users tools for 
developing own solution strategies to these kinds of problems.
APPENDIX P 
A  prerequisite  for  running  implicit  is  to  use  a  double  precision  version  of  LS-DYNA, 
and a machine with a significant amount of memory.  A theoretical overview of implicit 
can be found in the LS-DYNA Theory Manual implicittheorychapter. 
NONLINEAR IMPLICIT ANALYSIS 
Activating Implicit Analysis 
The  keyword  *CONTROL_IMPLICIT_GENERAL  is  used  to  activate  the  implicit 
method, and in principle it is sufficient to set  
IMFLAG = 1 
DT0 = some reasonable initial time step. 
The initial time step should be chosen small enough to resolve the frequency spectrum 
of  interest  and/or  provide  decent  convergence  properties,  but  large  enough  to  benefit 
from an implicit analysis.  With no other implicit options, this converts an explicit input 
deck to a static implicit input deck with a constant time step throughout the simulation 
and the problem will terminate upon convergence failure.  Time stepping strategies to 
prevent this are discussed Time Stepping Strategies 
Singularities and Eigenvalue Analysis 
The  first  concern  in  implicit  analysis  is  to  prevent  singularities  in  the  stiffness  matrix, 
otherwise  the  chance  of  succeeding  is  close  to  none.    The  major  source  to  a  singular 
stiffness matrix is the presence of rigid body modes in a static problem, and these can be 
revealed 
using 
*CONTROL_IMPLICIT_EIGENVALUE and putting 
eigenvalue 
analysis. 
done 
This 
by 
an 
in 
is 
NEIG = number of modes to extract. 
Run an eigenvalue analysis and extract (if practically possible) enough modes to see all 
the  rigid  body  modes  just  to  get  an  impression  of  the  properties  of  the  model.    The 
frequencies are in the output text file “eigout” and the mode shapes can be animated in 
the binary output file “d3eigv” using LS-PrePost.  Some rigid body modes may come as 
a surprise and should be constrained, a typical example of this are beams that are free to 
rotate around its own axis.  Other rigid body modes are a consequence of the nature of 
the problem and cannot be constrained without destroying the connection to reality, an 
example  of  this  could  be  components  that  are  to  be  constrained  with  contacts  but  are 
initially  free  to  move.   There  are  several  strategies  to  deal  with  these  latter rigid  body 
modes, some are discussed in the context of contacts but here dynamics is used.  
Dynamics and Intermittent Eigenvalue Analysis 
Dynamics 
*CONTROL_IMPLICIT_DYNAMICS by putting 
alleviates 
singular 
rigid  body  modes 
and 
is 
activated  on
APPENDIX P 
IMASS = 1 or a negative number. 
If the purpose is to solve a dynamic problem in the first place, then just use IMASS = 1 
and  don’t  bother  about  the  other  parameters,  otherwise  some  other  strategy  is 
necessary.  The idea is to get off to a start using dynamic analysis, and as the simulation 
gets  to  a  point  where  rigid  modes  have  been  constrained  by  contacts,  dynamics  is 
turned off.  The simplest way of doing this is to put 
TDYBIR = 0 
TDYDTH = time when contacts have been established and rigid body modes are 
constrained 
TDYBUR = time after TDYDTH for fading out dynamics between TDYDTH and 
TDYBUR. 
If the dynamic results are of no interest but just a way to proceed to the static solution, 
then it is recommended to use numerical damping to prevent unnecessary oscillations, 
i.e., put 
GAMMA = 0.6 
BETA = 0.38. 
This should be enough to start up most problems of interest.  A restriction with this is 
that  when  dynamics  has  been  turned  off  it  cannot  be  turned  on  again.    If  this  is 
necessary for some reason, then a negative number of IMASS should be used to control 
dynamics through a load curve. 
If  it  is  hard  to  deduce  how  to  choose  the  time  when  to  turn  off  dynamics,  the  use  of 
intermittent eigenvalues may be of great help.  By putting 
NEIG = a negative number 
on  *CONTROL_IMPLICIT_EIGENVALUE  the  user  may  extract  eigenvalues  at  given 
time points during a nonlinear simulation and deduce from that if all rigid body modes 
have been eliminated. 
The Geometric Stiffness Contribution 
Stiffness  singularities  may  also  occur  during  simulation  due  to  a  complex  global 
phenomenon  involving  the  stress  state  and  geometry.    For  instance  could  slender 
components with compressive stresses give rise to zero eigenvalues, commonly known 
as  buckling.    The  mathematical  explanation  to  these  kinds  of  singularities  is  that  the 
material  and  geometric  stiffness  contributions  cancel  out,  and  for  this  reason  the 
geometric contribution to the stiffness matrix is in LS-DYNA optional.  It is activated by 
putting
APPENDIX P 
IGS = 1 
on  *CONTROL_IMPLICIT_GENERAL. 
this 
contribution  have  a  negative  effect  on  convergence  although  it  sometimes  helps.    It  is 
recommended to leave this as default and turn it on if other strategies fail.  A controlled 
way of getting past singular points of this type is to use so called arc length methods for 
which the geometric stiffness should be turned on, this way of dealing with the problem 
is discussed in the Theory Manual arclengthchapter. 
  Most  often  singularities  due 
to 
BFGS or Full Newton 
The nonlinear solver parameters are set on *CONTROL_IMPLICIT_SOLUTION where 
the solver type is specified as 
NSOLVR = nonlinear or linear implicit analysis option 
By  default,  a  nonlinear  BFGS  solution  strategy  is  used  where  the  stiffness  matrix  is 
reformed every 11th iteration and a maximum of 15 reformations is allowed (for a linear 
solution set NSOLVR = 1).  These parameters are set by 
ILIMIT = iterations between reforming stiffness matrix 
MAXREF = maximum number of stiffness reformations 
on  *CONTROL_IMPLICIT_SOLUTION.    Reforming  the  stiffness  matrix  is  computa-
tionally  expensive  but  stabilizes  the  solution  procedure,  and  the  best  strategy  in  this 
context  is  very  much  problem  dependent.    The  recommendation  is  to  start  with  the 
default strategy and if necessary change them.  For hard problems decrease ILIMIT and 
for problems that converge well increase ILIMIT.  For really bad problems switch to full 
Newton (the safe bet) by for instance putting 
ILIMIT = 1 
MAXREF = 30. 
Keep the maximum number of reformations reasonably low or otherwise it may take an 
unnecessary amount of time just to reach convergence failure.  
Convergence 
Tolerances 
Convergence  is  based  on  changes  in  displacements,  energies  and  optionally  residual 
forces, and the tolerance levels are set by 
DCTOL = Relative displacement tolerance 
ment tolerance  
ECTOL = Relative energy tolerance 
tolerance 
DMTOL = Maximum 
displace-
EMTOL = Maximum 
energy
APPENDIX P 
RCTOL = Relative residual tolerance 
ABSTOL = Absolute tolerance 
RMTOL = Maximum residual tolerance 
on  *CONTROL_IMPLICIT_SOLUTION.    The  tolerances  on  the  left  are  based  on 
Euclidian  norms  of  the  involved  vectors,  whereas  the  ones  on  the  right  are  based  on 
maximum norms.  The maximum norm tolerances are optional and should be activated 
if increased accuracy is desired at the price of more implicit iterations.  To keep things 
simple, the discussion that follows pertains only to the Euclidian norm tolerances. 
By default, the progress of the equilibrium search is not shown to the screen but can be 
activated using 
NLPRINT = nonlinear output diagnostics 
input parameter.  The box below shows a typical iteration sequence, where the norms of 
displacement  and  energy  are  displayed.    When  these  norms  are  reduced  below  user 
prescribed tolerances (default 0.001 and 0.01, respectively), the iteration process is said 
to  have converged,  and  the  solution  proceeds  to  the  next time  step.    The  message  files, 
messag in SMP and mesXXXX in MPP, typically contain a whole lot more information 
that will be dealt with further in Output and Stretching for Convergence. 
 BEGIN static time step     3 
 ============================================================ 
                time =  1.50000E-01 
   current step size =  5.00000E-02 
 Iteration:   1     *|du|/|u| =  3.4483847E-01     *Ei/E0 =  1.0000000E+00 
 Iteration:   2     *|du|/|u| =  1.7706435E-01     *Ei/E0 =  2.9395439E-01 
 Iteration:   3     *|du|/|u| =  1.6631174E-03     *Ei/E0 =  3.7030904E-02 
 Iteration:   4     *|du|/|u| =  9.7088516E-05     *Ei/E0 =  9.6749731E-08 
Premature Convergence 
The  last  of  these  parameters  (ABSTOL)  overrides  the  other  three  (DCTOL,  ECTOL, 
RCTOL) in the sense that if the residual force is small enough, convergence is detected 
regardless  if  the  other  three  criteria  are  fulfilled  or  not.    It  has  been  seen  that  this 
sometimes  give  rise  to  so  called  premature  convergence,  converged  states  are  not  really 
converged in the sense that the residual norm is small enough.  This gives bad results 
and it is usually recommended to tighten this tolerance to 10−20 to prevent this.  On the 
other hand, if the problem is very hard this may prevent convergence to the extent that 
going  back  to  the  default  is  more  or  less  necessary.    It  is  difficult  to  give  a  general 
recommendation that holds for every problem. 
As  for  the  other  three  parameters,  the  one  that  usually  comes  into  practice  is  the 
displacement criterion DCTOL.  The energy criterion ECTOL is often easy to fulfill and 
the residual criterion is disabled by default and there may be no reason to activate this 
(that  is  unless  a  completely  Using  Residual  Tolerance  is  used,  or  if  Stretching  for 
Convergence  arise).    Using  the  default  values  on  all  three  is  usually  good  enough  to 
give  acceptable  results  in  decent  time.    For  problems  with  poor  convergence,  the 
question  of  tightening  or  relaxing  these  parameters  (that  is  the  displacement
APPENDIX P 
convergence  criterion)  is  up  for  debate.    It  is  tempting  to  believe  that  relaxing  the 
constraints  will  give  better  convergence  which  may  or  may  not  be  true.    Sloppy 
convergence  criteria  may  once  again  result  in  premature  convergence,  and  this  will 
have  a  negative  effect  on  the  subsequent  steps.    The  general  recommendation  would 
have to be to leave these unchanged, and be aware that relaxing them may not result in 
getting further in the implicit simulation. 
Using Residual Tolerance 
A novel strategy that seems to make sense and works well for some problems is to only 
use  tolerances  on  residual  forces  RCTOL.    This  relies  much  on  that  the  degree  of 
nonlinearity  of  the  simulation  model  is  moderate,  but  it  could  be  well  worth  trying.  
The first thing to do would be to put DCTOL and ECTOL to large numbers to disable 
them  and  put  RCTOL  to  a  relatively  small  number,  start  with  0.01  and  see  how  that 
works  out.    This  must  be  complemented  with  an  absolute  tolerance  on  the  residual 
forces  to  get  past  the  initial  stages  where  the  residual  forces  are  small  enough  to  not 
fulfill  the  relative  tolerance.    This  is  done  by  putting  ABSTOL  to  a  negative  number, 
which  is  a  different  absolute  criterion  compared  to  putting  it  to  a  positive  number.  
Now, this number is very problem dependent as this says that convergence is attained 
as soon as the Euclidian norm of the residual force vector is smaller than the absolute 
value  of  ABSTOL.    It  goes  without  saying  that  this  require  running  the  problem  for  a 
few  steps  to  monitor  the  residual  norm  in  the  message  files  as  described  below,  this 
should give an indication on how to determine the ABSTOL value. 
Convergence Norms 
The degrees of freedom encountered in an LS-DYNA simulation are either translational 
or rotational, where the latter comes from the presence of beams and shells.  Historically, 
convergence  check  is  on  norms  of  the  translational  degrees  of  freedom  only,  which  is 
unsettling from the fact that rotational residual forces (moments) are equally important 
in an implicit simulation.  It is therefore recommended to use 
NLNORM = choice of convergence norms 
on  *CONTROL_IMPLICIT_SOLUTION  to  change  this  default  (which  is = 2).    While 
NLNORM = 3  will  incorporate  residual  degrees  of  freedom  separately  and  is  a  more 
satisfying  approach,  the  recommended  option  is  to  use  NLNORM = 4  or  NLNORM  a 
negative  number.    NLNORM = 4  will  treat  the  entire  force  and  displacement  vector, 
respectively,  as  one  complete  mathematical  vector  and  the  convergence  norms  and 
scalar products used for checks are simply the Euclidian norms of these vectors.  This 
will  make  the  energy  norm  unit  consistent  since  each  term  in  the  scalar  product  is  an 
energy  quantity,  either  through  force  times  displacement  or  moment  times  angular 
increment.    The  displacement  norm  and  residual  norm,  however,  contains  a  mix  of 
translational and rotational quantities which means that displacements are summed to 
angular  increments  and  forces  are  summed  to  moments.    This  is  of  course  not  pretty, 
but  it  can  be  interpreted  as  using  a  length  scale  of  1  for  the  rotational  degrees  of 
freedom,  meaning  that  displacements  are  summed  to  1  length  unit  times  angular
APPENDIX P 
increments, and moments are summed to 1 length unit times forces.  If the model is in 
length  units  of  𝑚𝑚,  and  the  element  sizes are  in  the  order  of 1 𝑚𝑚,  this  seems  to  be  a 
reasonable length scale.  But if the length unit is something else, it is convenient to use 
NLNORM = -(length  scale)  to  scale  with  the  number  that  corresponds  to  1 𝑚𝑚.    If  for 
instance the length unit is 𝑚, then NLNORM = -0.001 is presumably a reasonable choice. 
Time Stepping Strategies 
By default, LS-DYNA will terminate when a step fails to converge.  This is unfortunate 
since it may just be that the step is too large to achieve convergence and taking smaller 
steps would solve this problem.  Instead of starting all over with a smaller step size, set 
IAUTO = 1 to activate automatic time stepping 
on *CONTROL_IMPLICIT_AUTO.  When the problem fails to converge LS-DYNA will 
with this option go back to the previously converged state and retry with a smaller step 
size.  If the problem converges well, the step size is increased for subsequent steps.  This 
process  of  backing  up  and  retrying  difficult  steps  lends  much  persistence  to  the 
analysis, and is often the only procedure for solving highly nonlinear problems short of 
adjusting the step size manually and the recommendation is to always turn automatic 
time stepping on. 
Another parameter worth mentioning in this context is 
DTMAX = Max time step allowed, or a negative number 
on the same card.  This is the maximum step size possible and should be chosen so as to 
not  loose  necessary  information  in  the  results,  i.e.,  be  sure  to  resolve  frequencies, 
contacts and nonlinear material response to a satisfactory degree.  A negative value of 
this parameter will give the maximum step size as a function of the simulation time and 
also allows for hitting key points that are of interest.  The user may for instance look for 
the  peak  stress  for  a  certain  external  load  and  hitting  the  point  in  time  when  this 
happens  is  crucial.    It  also  allows  for  taking  smaller  steps  during  critical  stages  in  the 
simulation without wasting resources away from these stages. 
Line Search 
A good line search strategy is crucial in solving nonlinear implicit problems, without it 
only simple problems would be solvable.  There are a few line search options available 
and these are activated by 
LSMTD = Line search method 
on *CONTROL_IMPLICIT_SOLUTION.  The default method is based on minimizing a 
potential  energy  along  the  search  direction  and  at  the  same  time  keeping  track  of  the 
residual  force  magnitude.    It  also  detects  when  a  BFGS  step  results  in  negative  initial 
energy and the stiffness matrix is reformed for robustness (this can only happen when
APPENDIX P 
the  stiffness  matrix  has  negative  eigenvalues),  and  even  suppresses  the  occurrence  of 
negative  volumes.    Line  search  type  2  is  based  on  residual  forces  and  is  more  robust 
than  the  others,  the  drawback  is  that  it  typically  results  in  too  small  steps  and  is  not 
practically  useful.    Line  search  type  3  is  very  similar  to  type  4,  but  is  not  tracking  the 
residual  force  or  avoids  negative  volumes  to  the  same  extent,  and  in  sum  there  is  no 
practical reason for choosing methods 1 through 3.  Worth mentioning is however line 
search type 5 which combines the energy and residual method in a stricter sense.  That 
is, it minimizes the potential energy just like type 4 but it only allows the residual norm 
to double at each implicit iteration.  This has shown to be robust but on the other hand 
slow  in  convergence  and  is  to  be  used  for  problems  that  have  difficulties  to  converge 
with  the  default  line  search  strategy.    This  has  had  a  huge  impact  on  the  treatment  of 
rubber models for instance.  An interesting combination is to use line search method 5 
together with the strategy of converging based onUsing Residual Tolerance. 
Finally, the line search tolerance  
LSTOL = Line search tolerance 
on *CONTROL_IMPLICIT_SOLUTION is fine as it is, don’t change it. 
Output 
As previously mentioned, the output to the message file is more extensive than that to 
the  screen/stdout.    To  novice  or  average  implicit  users  this  information  may  be  more 
than can be digested at first and this section may be LINEAR EQUATION SOLVER, but 
with  experience  the  output  can  become  really  useful  when  running  into  convergence 
issues.    For  this  discussion  it  is  important  to  distinguish  between  different  types  of 
iterations, and we use the term time/load step to mean the actual advance in simulation 
time, implicit iteration to indicate points in the iterative solution procedure where a new 
search  direction  is  obtained  (corresponding  to  either  Newton  or  BFGS)  and  line  search 
iteration  to  indicate  the  search  for  an  optimal  step  size  along  a  given  search  direction.  
We begin by showing a typical iteration output for when NLPRINT = 3 following by a 
bulletin list explaining the content. 
1BEGIN implicit dynamics step      2 t = 2.5849E-01 
 ============================================================ 
                time =  2.58489E-01 
   current step size =  1.58489E-01 
. 
. 
. 
2Newton step computed 
 Initial translational energy =  1.4031740E-01 
3Initial total energy         =  1.4031740E-01 
 Initial residual norm        =  7.5755334E-01 
4Translational nodes norm     =  7.1314670E-01 
 Translational nodes max      =  1.9159278E-01 at node         440788 
 Translational rigid body norm =  3.5324028E-03 
 Translational rigid body max =  2.3897586E-03 at body        4000024
APPENDIX P 
 Rotational rigid body norm   =  2.5553155E-01 
 Rotational rigid body max    =  1.7834357E-01 at body        4000024 
5Evaluated residual for full step 
 Current translational energy =  9.0141343E-02 
6Current total energy         =  9.0141343E-02 
 Current residual norm        =  2.2038666E+00 
 Translational nodes norm     =  2.1950775E+00 
 Translational nodes max      =  1.0295509E+00 at node         440984 
 Translational rigid body norm =  3.4677960E-02 
 Translational rigid body max =  2.6701145E-02 at body        4000024 
 Rotational rigid body norm   =  1.9354585E-01 
 Rotational rigid body max    =  1.2669458E-01 at body        4000024 
7Evaluated residual for step size  6.6666667E-01 
 Current translational energy =  1.1123844E-01 
 Current total energy         =  1.1123844E-01 
 Current residual norm        =  1.5007375E+00 
 Translational nodes norm     =  1.4922142E+00 
 Translational nodes max      =  7.1187918E-01 at node         440984 
 Translational rigid body norm =  1.6121536E-02 
 Translational rigid body max =  1.2659274E-02 at body        4000024 
 Rotational rigid body norm   =  1.5890244E-01 
 Rotational rigid body max    =  1.0852930E-01 at body        4000024 
 Evaluated residual for step size  3.3333333E-01 
 Current translational energy =  1.2543971E-01 
 Current total energy         =  1.2543971E-01 
 Current residual norm        =  8.3754668E-01 
 Translational nodes norm     =  8.1775945E-01 
 Translational nodes max      =  3.0290699E-01 at node         440984 
 Translational rigid body norm =  5.4770134E-03 
 Translational rigid body max =  4.5377150E-03 at body        4000024 
 Rotational rigid body norm   =  1.8089755E-01 
 Rotational rigid body max    =  1.2913973E-01 at body        4000024 
 Line search continues 
 Max relative step            =  0.3499001E+00 
8Lower bound                  =  3.3333333E-01 
 Upper bound                  =  1.0000000E+00 
 Evaluated residual for step size  7.7777778E-01 
 Current translational energy =  1.0487486E-01 
 Current total energy         =  1.0487486E-01 
 Current residual norm        =  1.7421066E+00 
 Translational nodes norm     =  1.7342352E+00 
 Translational nodes max      =  8.2830775E-01 at node         440984 
 Translational rigid body norm =  2.1464316E-02 
 Translational rigid body max =  1.6693623E-02 at body        4000024 
 Rotational rigid body norm   =  1.6402030E-01 
 Rotational rigid body max    =  1.0799892E-01 at body        4000024 
 Evaluated residual for step size  5.5555556E-01 
 Current translational energy =  1.1674955E-01 
 Current total energy         =  1.1674955E-01 
 Current residual norm        =  1.2575584E+00 
 Translational nodes norm     =  1.2472759E+00 
 Translational nodes max      =  5.8455890E-01 at node         440984 
 Translational rigid body norm =  1.1655353E-02 
 Translational rigid body max =  9.2884622E-03 at body        4000024
APPENDIX P 
 Rotational rigid body norm   =  1.6006264E-01 
 Rotational rigid body max    =  1.1222751E-01 at body        4000024 
9Line search converged in    2 iterations 
10Max relative step            =  7.1106671E-01 
11Iteration:    5    displacement             energy               residual 
 ----------           not conv.              not conv.           converged 
 norm ratio           1.013E+00              1.000E+00              n/a        
 current norm         8.446E-01              1.403E-01           1.258E+00 
 initial norm         8.338E-01              1.403E-01           7.575E+00 
-------------    trans       rot      trans      rot        trans       rot 
max  node  norm      8.533E-02    0.000E+00    2.052E-02    0.000E+00    5.846E-01  
0.000E+00 
   at node ID   4000674    9007526     440984    9007526     440984    9007526 
------------- 
       RB max   3.449E-02  6.613E-04 -5.507E-04  7.681E-05  9.288E-03  1.122E-
01 
     at RB ID   4000024    4000024    4000024    4000024    4000024    4000024  
Referring  to  the  superscripts  at  the  beginning  of  the  lines  in  the  excerpt  above,  and 
taking them in order of appearance, we have at 
1.Beginning a dynamic implicit time/load step, the goal is to get to a given time point 
(in  this  case  2.5849E-01  using  a  step  size  of  1.58489E-01).    Implicit  time/load 
steps are either dynamic, static or semidnmc, where the last one indicates a transi-
tion phase between dynamics and statics. 
2.A  Newton  implicit  iteration  is  performed,  meaning  that  a  full  reformation  of  the 
stiffness  matrix  has  just  been  made.    Other  implicit  iterations  can  be  either  a 
linear if at the first iteration of a time/load step, or BFGS if the implicit iteration 
corresponds to a quasi-Newton step. 
3.Initial  norms  are  displayed  at  the  beginning  of  each  implicit  iteration,  these 
numbers are used as reference for the line search algorithm when checking line 
search convergence. 
4.Detailed  initial  norms  are  displayed,  separating  out  translational/rotational  as 
well  as  nodal/rigid  body  Euclidian/max  norms.    The  node  number  and  rigid 
body attaining the global maximum norms are displayed and can be used to spot 
critical points in the model, in this particular case node 440984 and part 4000024 
would be the likely candidates to trouble. 
5.A full step along the search direction is taken, as a candidate for the next implicit 
iteration. 
6.Norms for the full step is displayed, the line search algorithm compares these with 
the ones from 3 to deduce if line search convergence criterion is fulfilled. 
7.Line  search  is  in  this  case  needed,  and  information  for  further  iterates  along  the 
search direction is displayed in analogy to previous line search iterates.  If no line 
search  had  been  needed,  the  string  Line  search  is  skipped  would  have  been  dis-
played. 
8.The  way  line  search  is  performed,  each  line  search  iteration  narrows  in  on  the 
optimal step and the bounds within which the optimal step is sought is continu-
ously  displayed.    The  size  of  this  interval  becomes  smaller  and  smaller  with
APPENDIX P 
increasing number of line search iterations, but convergence should preferably be 
attained before it tends to zero. 
9.Line  search  converged  here  in  2  iterations;  as  a  rule  of  thumb  the  number  of 
iterations for line search should be about 10 or less.  For critical steps one might 
accept  20  iterations  but  that  should  be  among  the  exceptions.    If  the  string  Line 
search  did  not  converge  is  displayed,  that  is  an  indication  of  something  being 
terribly wrong. 
10.After each implicit iteration, Max relative step indicates how large steps have been 
taken during line search so  far.  It also indicates how well prescribed motion is 
approximated where a value of 1 is perfect.  For values below 1 and in the pres-
ence  of  non-zero  prescribed  motion,  convergence  will  not  be  accepted  even 
though  all  norms  are  within  prescribed  tolerances.    This  will  instead  issue  the 
warning Convergence prevented due to unfulfilled boundary conditions and iterations 
continue. 
11.Diagnostics  for  iteration  5  is  displayed,  similar  numbers  as  shown  during  line 
search  but  in  another  format.    Furthermore,  the  initial  norms  here  refer  to  the 
initial norms from the beginning of the implicit time/load step and not from the 
beginning  of  the  implicit  iteration.    This  table  can  be  used  to  deduce  how  close 
the  implicit  time/load  step  is  at  converging.    The  single  important  number  for 
comfortably  assessing  the  accuracy  of  an  implicit  iterate  is  the  residual  norm, 
currently  displayed  as  1.258E+00  (bold-faced  in  the  table),  since  this  should  be 
small for good results. 
At equilibrium, the output ends with a summary on how convergence was achieved.  It 
may look like 
Convergence detected as a combination of 
1.Ratio of euclidian displacement 
Value =   2.3417E-03 vs Tolerance =  2.5000E-3 
2.Ratio of euclidian energy 
Value =   3.2269E-08 vs Tolerance =  1.0000E-2 
which tells us that the ratio of displacement was below DCTOL = 2.5E-3 and the ratio of 
energy was below ECTOL = 1E-2.  If other criteria are satisfied, these will be listed too. 
So, with NLPRINT = 3 information from every force evaluation is given, including type 
of step taken, the line search step size, the potential energy value used in line search and 
the  magnitude  of  the  residual  force.    A  point  is  made  here,  already  Premature 
Convergence and will be repeated, and it is the following.  The nonlinear implicit solver 
is solving for zero residual force, so basically the number observed for the magnitude of 
the  residual  force  should  be  small  upon  convergence  (bold-faced  in  the  table).    If  it  is 
not,  then  the  convergence  is  premature  and  the  results  may  not  be  correct  and 
subsequent steps are in danger.  What “small” means in this context is hard to say since 
this depends on units as well as loads and geometry of the problem, but a good sign is 
that the residual force does not grow by more than the external loads in the problem do.  
Another  thing  to  observe  is  how  the  Line  Search  is  doing,  if  the  line  search  starts
APPENDIX P 
needing many iterations and very large variations in the residual force along the search 
direction  is  observed,  then  it  is  likely  that  something  in  the  model  is  causing  this 
behavior.    A  safe  bet  is  that  contact  states  are  changed  along  the  line  search  direction 
causing discontinuities in the residual force and indicates that some remodeling has to 
be done. 
We  will  come  back  to  this  section  when  discussion  Taking  Advantage  of  ASCII 
Information and strategies to prevent them. 
LINEAR EQUATION SOLVER 
General 
Within  each  equilibrium  iteration,  a  linear  system  of  equations  of  the  form  𝑲𝛥𝒖 = 𝑹 
must be solved.  To do this, the stiffness matrix 𝑲 is factorized and applied to the out-
of-balance  load  or  residual  𝑹,  yielding  a  displacement  increment  𝛥𝒖.    Storing  and 
solving this linear system represents a large portion of the memory and CPU costs of an 
implicit  analysis.    LS-DYNA  uses  a  multi-frontal  sparse  direct  solver  and  nested 
dissection,  and  for  a  problem  with 𝑁  number  of  nodes,  the  number of  operations  and 
memory  storage  is  asymptotically  proportional  to  𝑁3/2  and  𝑁𝑙𝑜𝑔𝑁,  respectively.    This 
should  give  a  ballpark  indication  on  the  growth  when  increasing  the  size  of  a  given 
model.  It must be stressed however that it is a priori difficult to predict the actual value 
of these numbers as they are highly dependent on the problem solved, in particular on 
the  nodal  connectivity  through  elements  and  contacts.    In  the  end  we  are  left  at 
qualitative  guessing  how  to  set  memory  flags  or  determining  model  size  in  order  to 
push the limits for a given computer architecture. 
We here focus on the memory, and the purpose is twofold.  First it is a documentation 
of  the  memory  diagnostics  that  is  written to  the  output  message  files  (messag  in  SMP 
and mesXXXX in MPP) of LS-DYNA for the linear solvers.  The level of information is 
regulated by the 
LPRINT = Linear solver diagnostics level 
input  parameter  on  *CONTROL_IMPLICIT_SOLVER,  and  this  text  will  cover 
LPRINT = 2  as  the  information  for  higher  values  is  of  no  particular  interest  to  others 
than  developers.    Second  it  should  help  understanding  the  interrelationship  between 
the  size  of  a  model  and  the  memory  required  to  obtain  a  solution.    We  emphasize 
however that different classes of problems most likely require different guidelines (shell 
and  solid  structures  typically  result  in  different  matrix  topologies  for  instance)  and  to 
this end the user is left at earning this experience on his own. 
Memory 
The memory is specified and reported in terms of words, where 1 word is equivalent to 4 
bytes in single precision and 8 bytes in double precision arithmetic.  To simplify things,
APPENDIX P 
a word can in this context be seen as the equivalent of a real number or an integer.  For 
implicit  calculations  the  executable  used  is  typically  double  precision,  so  to  convert 
from words to bytes one needs to multiply by 8. 
In  starting  a  simulation  the  user  typically  specifies  the  static  memory,  for  instance  in 
SMP 
ls-dyna i = in.k memory = 200m 
meaning  that  LS-DYNA  tries  to  allocate  200  Mwords  for  storing  most  of  the  data.    In 
MPP,  the  physical  memory  is  distributed  among  processes  and  this  option  applies  to 
each individual process.  In MPP there is also an option to add a second memory flag, 
for instance 
mpp-dyna i = in.k memory = 1000m memory2 = 200m 
and  this  means  that  200  Mwords  are  allocated  for  each  process  while  1000  Mwords  is 
allocated on the first process to handle everything up to the point when the model data 
has  been  distributed  among  all  the  involved  processes.  The  memory  size  may  also  be 
specified on *KEYWORD. For implicit it is recommended to avoid memory2 in order to keep 
the memory balance between processors. 
When a certain feature requires a slot in the memory, this is reported in the output text 
files, for instance as 
contracting memory to    2306940 implicit friction 
expanding   memory to    2306955 joints 
In the example above, the memory pointer after having allocated for implicit friction is 
at 2306940 and joints reserves 15 words and increment the memory pointer accordingly.  
So the memory used up to this point is roughly 2.3 Mwords for this particular process.  
At the end of the initialization a memory report is written and can look like 
S t o r a g e  a l l o c a t i o n 
Memory required to begin solution      :    2680153 
Linear Alg dynamically allocated memory:     880685 
Additional dynamically allocated memory:    1553130 
                                  Total:    5113968 
The  total  amount  of  memory  used  up  to  this  point  is  roughly  5.1  Mwords,  which  is 
partitioned in the static memory specified and dynamic memory that is allocated on the 
fly so to speak, typically if a certain amount of memory needed cannot be estimated in 
due time to adequately include it in the static chunk of memory.  Whenever a memory 
violation  occurs,  for  instance  when  trying  to  allocate  more  memory  than  physically 
available  or  if  more  memory  needs  to  be  specified,  LS-DYNA  terminates  with 
appropriate  error  information.    The  static  memory  for  the  linear  solver  is  allocated 
thereafter, which is the topic for the next section.
APPENDIX P 
Linear Solver Memory Consumption 
For LPRINT = 2, some memory information is given in the output files, and this is here 
presented in order of execution, thus as they appear in the files.  We repeat that this is 
the  information  obtained  in  the  message  files  and  is  thus  referring  to  the  memory 
consumption  for  this  particular  process  if  MPP  is  considered.    For  the  sake  of 
completeness  we  also  cover  the  diagnostics  related  to  the  CPU  time  for  the  involved 
stages in the linear solution. 
First the memory required for handling constraints is reserved and is reported as 
expanding   memory to    2893375 implicit lsolvr allocation 1 
After  this  memory  is  reserved  for  symbolic  factorization,  which  is  performed  prior  to 
the  actual  solve  to  predict  the  storage  requirement  for  the  factorized  system  matrix.  
This allocation is reported as 
expanding   memory to    7639758 implicit matrix storage 
Also, some memory is reserved for the sparse matrix, including index pointers to non-
zero elements, and is reported as 
expanding   memory to   15077248 linear eqn.  solver allocation 2d 
Here the last information (2d) is referring to the solver used and may change depending 
on user options. 
Before the symbolic factorization takes place, current information on the system matrix 
and workspace reserved for implicit is reported 
local number of rows      =              68490 
local size of matrix      =            2338945 
local len of workspace    =           15077248 
ptr to start of wrkspc    =            2893375 
The first number refers to the number of independent degrees of freedom in the model, 
i.e., the number of rows in the system matrix, and the second to the number of nonzero 
entries    before  factorization  takes  place,  i.e.,  after  assembly.    The  third  row  of 
information  is  somewhat  misleading  as  this  is  actually  the  total  amount  of  memory 
reserved  and  not  the  size  of  the  workspace  itself.    The  workspace  here  means  the 
memory  reserved  for  the  linear  solution,  and  its  size  is  obtained  by  subtracting  the 
pointer to start of workspace and the local length of workspace. 
The  symbolic  factorization  is  now  performed  and  information  on  the  CPU  time  for 
doing this together with the estimated size of the factorized matrix is reported 
CPU: symbolic factor     =          0.200 
WCT: symbolic factor     =          0.203 
storage currently in use =        1038915
APPENDIX P 
storage needed           =       12913838 
factor speedup           =     1.9197E+00 
solve  speedup           =     1.9378E+00 
est.  factor nonzeroes    =     5.1432E+07 
est.  factor operations   =     1.2099E+11 
est.  total factor nz.    =     9.9666E+07 
est.  max.  factor op.    =     1.2099E+11 
est.  total factor op.    =     2.3293E+11 
est.  max.  factor nz.    =     5.1432E+07 
The  first  two  rows  reports  the  CPU  and  wall  clock  time  for  doing  the  symbolic 
factorization  in  terms  of  seconds.    The  next  two  are  storage  requirements  for  the 
symbolic factorization, of which the latter is the memory reserved for this.  After this we 
have estimations of the speedup in the factorization and subsequent solve of the linear 
system  of  equations,  this  is  a  report  from  an  MPP  run  on  2  processors.    The  last  lines 
refer  to  the  estimated  requirement  for  storing  and  factorizing  the  system  matrix,  and 
distinguish between the local, total and maximum number of each of these two entries.  
This allows for determining the memory scaling in the case of an MPP run. 
Now LS-DYNA is in the position of reserving space for the factorization of the system 
matrix, and a report on the storage needed for this is given. 
symbolic storage       1 =           1038915 
in-core numeric storg  1 =          62762269 
out-of-core num.  storg 1 =          13168676 
symbolic         storg 1 =              1.04 Mw 
in-core numericl storg 1 =             69.06 Mw 
out-of-core num.  storg 1 =             14.51 Mw 
Here basically the same information is repeated, except for a slight increment in order 
to account for potential penalty when doing the actual factorization.  The first is again 
the memory reserved for the symbolic factorization and the other two are the memory 
required  to  perform  an  in-core  and  out-of-core  factorization,  respectively.    If  the 
memory  available  is  not  sufficient  for  doing  an  in-core  factorization,  LS-DYNA  warns 
about  this  and  attempts  to  do  an  out-of-core  factorization,  which  means  that  the  hard 
disk  is  used  to  store  information  during  factorization.    If  this  warning  appears  it  is 
recommended  to  restart  the  simulation  and  using  more  memory  since  out-of-core 
significantly  (writing  to  disk  is  more  expensive  than  accessing  memory)  adds  to  the 
wall  clock  time  for  solving  the  problem.    If  the  memory  for  doing  an  out-of-core 
factorization is insufficient, LS-DYNA will terminate with an error message.  Otherwise, 
memory is reserved and reported 
expanding   memory to  77737167 linear eqn.  solver numerical phase 1 
meaning that the total amount of memory reserved at this point is roughly 78 Mwords. 
At  this  point  a  redistribution  of  the  system  matrix  is  performed  and  a  short  report  is 
given on this
APPENDIX P 
symbolic storage       2 =           1038915 
in-core numeric storg  2 =          68238926 
out-of-core num.  storg 2 =          11553502 
Now  the  actual  factorization  takes  place  and  a  report  from  this  is  given  where  the 
information of interest is 
CPU: factorization       =            59.025 
WCT: factorization       =            50.151 
act.  factor nonzeroes    =        5.1236E+07 
act.  factor operations   =        1.2092E+11 
act.  max.  factor nz.    =        5.1236E+07 
act.  max.  factor op.    =        1.2092E+11 
act.  total factor nz.    =        9.9666E+07 
act.  total factor op.    =        2.3293E+11 
which basically is the  same information as from the symbolic  factorization except that 
now it is the actual instead of the estimated values that is reported. 
Finally, the forward and backward substitutions are allocated for and performed.  The 
information given is 
symbolic storage       3 =           1038915 
in-core numeric storg  3 =          68299122 
out-of-core num.  storg 3 =          16476693 
CPU: numeric solve       =             0.191 
WCT: numeric solve       =             0.194 
Concluding, the wall clock time for solving the system of linear equations is reported 
WCT: total imfslv_mf2    =            75.079 
ELEMENTS AND MATERIALS 
Implicit Accuracy 
Implicit  and  explicit  analysis  differ  in  many  respects,  an  important  one  is  that  the 
deformation during a single step is much larger in implicit than a typical one in explicit.  
In the context of elements and materials, the demand for stronger objectivity and higher 
accuracy in implicit is obvious.  The notion of implicit executing the same algorithms as 
a corresponding explicit analysis is whence not adopted in general.  This can optionally 
be further extended, using 
IACC = 1 to increase implicit accuracy 
on  *CONTROL_ACCURACY  will  make  selected  elements  strongly  objective  and 
enhance  the  accuracy  for  selected  materials.    For  instance  will  finite  rotations  be 
represented exactly and fully iterative plasticity adopted.  In addition, the flag applies 
to  tied  contacts  as  will  be  elaborated  on  below.    Currently  the  following  elements  are 
supported for this option
APPENDIX P 
Solid elements -2,-1,1,2 
Shell elements 4,-16,16,23,24 
Beam elements 1,2,9 
and materials 24 and 123 use fully iterative plasticity. 
CONTACTS 
Contacts  are  probably  among  the  hardest  features  to  treat  in  a  nonlinear  implicit 
simulation.    They  are divided  into  the  categories  tied  (bilateral)  and  sliding  (unilateral) 
contact,  and  the  characteristics  of  the  two  are  quite  different.    Tied  contacts  are  most 
often applied as constraints, only sometimes using a penalty formulation, and are fairly 
easy to deal with as they are only moderately nonlinear.  In contrast, sliding contacts are 
exclusively  implemented  as  penalty  contacts  and  hard  to  deal  with  because  of  the 
unilateral  condition.    While  the  number  of  contacts,  see  *CONTACT,  in  LS-DYNA  is 
abundant,  we  will  here  only  present  the  few  contacts  that  make  most  sense  to  use  in 
implicit. 
Tied Contacts 
Tied  contacts  in  implicit  analysis  should  be  accompanied  with  the  Implicit  Accuracy 
option,  as  this  essentially  reduces  the  number  of  relevant  contacts  to  use  to  only  six.  
These six contacts are 
*CONTACT_TIED_NODES_TO_SURFACE 
*CONTACT_TIED_NODES_TO_SURFACE_CONSTRAINED_OFFSET 
*CONTACT_TIED_NODES_TO_SURFACE_OFFSET 
*CONTACT_TIED_SHELL_EDGE_TO_SURFACE 
*CONTACT_TIED_SHELL_EDGE_TO_SURFACE_CONSTRAINED_OFFSET 
*CONTACT_TIED_SHELL_EDGE_TO_SURFACE_BEAM_OFFSET 
The  first  and  fourth  of  these  project  the  nodes  on  the  slave  side  to  the  master  surface, 
while the rest are offset contacts for which nodes will remain in place.  The fourth, fifth 
and  sixth  constrain  rotations  while  the  others  do  not.    The  third  and  sixth  are  penalty 
based,  while  the  others  are  constraint  based.    In  sum,  these  six  contacts  cover  most 
reasonable scenarios. 
The  implicit  accuracy  option  will  in  this  context  make  these  six  tied  contact  strongly 
objective,  and  built-in  intelligence  will  detect  whether  nodes  contain  rotations  to 
constrain or not.  A nice feature with the latter is that torsion is automatically applied 
with physical consistency, so it is for instance no problem to use single beams to model 
spotwelds  between  solid  elements,  and  when  using  the  same  connection  technique 
between shells the beam axial rotational degrees of freedom will be constrained to the
APPENDIX P 
translational  degrees  of  the  shells  and  thus  avoiding  the  relatively  weak  (and  non-
physical) drilling degree of freedom.  This situation is depicted below. 
be 
The choice of contact depends on the situation, but from a conceptual point of view it 
should 
use 
for 
*CONSTRAINED_TIED_SHELL_EDGE_TO_SURFACE_CONSTRAINED_OFFSET 
most  cases.    The  only  problem  then  would  be  if  complicated  geometry  results  in 
termination  due  to  overconstraining,  for  which  a  switch  to  the  corresponding  penalty 
is 
version 
motivated.  See remarks in the LS-DYNA keyword manual for more information. 
*CONSTRAINED_TIED_SHELL_EDGE_TO_SURFACE_BEAM_OFFSET 
ok 
to 
Sliding Contact 
The  choice  of  contact  in  this  section  is  the  Mortar  contact  as  this  seems  to  be  best 
implicit  contact  algorithm  when  considering  a  combination  of  speed,  accuracy  and 
robustness.    The  Mortar  contact  features  smoothness  and  continuity  that  is  highly 
appreciated  in  implicit  analysis,  but  is  on  the  other  hand  expensive  enough  to  not  be 
recommended  for  explicit  analysis.    Many  other  contact  algorithms  are  supported  for 
implicit analysis and execute faster than the Mortar contact, but this is often seen when 
the  infamous  IGAP  flag  is  set  to  default.    This  flag  manipulates  the  stiffness  matrix  to 
the  extent  that  accuracy  may  be  deteriorated,  and  if  used  the  results  should  be 
thoroughly  checked.    For  Mortar  contact  IGAP  has  a  different  meaning  as  will  be 
described IGAP.  See remarks in the LS-DYNA keyword manual for more information. 
Basics 
The  Mortar  contact  is  activated  by  typically  appending  the  suffix  MORTAR  to  the 
automatic  single  surface,  automatic  surface  to  surface  or  forming  surface  to  surface 
keywords.    It  can  also  be  run  as  tied  and  tiebreak  contacts.    All  Mortar  contacts  are 
segment  to  segment  and  penalty  based  and  the  tied  and  tiebreak  contacts  are  always 
offset, i.e., the tie occurs on the outer surfaces of shells and not on the mid surfaces.  For 
automatic  contacts,  edge  contact  with  flat  edges  is  always  active.    At  this  point,  it 
possesses features that are of particular interest to implicit and that are not available for 
other  contacts.    It  is  supported  in  both  SMP  and  MPP  but  the  option  MPP  does  not 
apply, and the SMP ignore flag applies.  The SOFT flag does not apply, to summarize it 
is a contact algorithm especially intended for implicit analysis. 
Recommendations
APPENDIX P 
For the forming contact the rigid tools must be meshed so that the normals are directed 
towards the blank, and contacts from above and below  must be separated into two or 
more  interfaces  because  contact  can  only  occur  from  one  side  of  the  blank  for  a  given 
contact  interface.    For  the  forming  contact,  rigid  shells  on  the  master  side  have  no 
contact  thickness.    This  is  not  the  case  for  automatic  contacts,  here  there  are  no 
restrictions  on  the  mesh  and  even  rigid  shells  have  contact  thickness.    For  all  Mortar 
contacts, part or part set based slave and master sides are recommended although not 
mandatory.    If  the  two  sides  in  the  contact  interface  have  different  stiffness,  use  the 
weak part as slave in order to get the best possible implicit convergence behavior.  This 
is automatically taken care of in a single surface contact. 
Characteristics 
The contact pressure in the Mortar contact is a parabolic function of the penetration in 
combination with a cubic stiffening phase.  In short, the contact stiffness depends on the 
slave  side  material  and  a  characteristic  length  of  the  slave  side  segment.  The 
characteristic length is for shells the shell thickness and for solids it is a median of the 
edges in the slave side of the contact interface, and the maximum penetration allowed is 
given as 95% of the average characteristic lengths on master and slave sides.  For solids 
the  definition  of  the  characteristic  length  may  have  the  consequence  that  the  stiffness 
becomes unnecessarily high if some elements are much smaller than most, and stiffness 
adjustments  may  be  necessary.    Furthermore,  the  characteristic  length  also  determines 
the maximum penetration as well as the search radius for finding contact pairs, for this 
reason the characteristic length can optionally be increased by assigning it on PENMAX 
on  optional  card  B.    In  most  cases  it  is  expected  that  default  value  (=0.0)  for  this 
parameter will suffice. 
IGAP 
The contact stiffness is parabolic with respect to penetration up to a penetration depth 
corresponding  to  half  of  the  maximum  penetration.    For  IGAP = 1  it  will  remain 
parabolic  for  even  larger  penetrations  but  the  user  may  increase  IGAP  which  means
APPENDIX P 
that the contact will stiffen for larger penetrations, in fact it will become cubic according 
to  the  picture  above.    The  purpose  of  increasing  IGAP  could  be  to  prevent  the 
penetration  from  becoming  larger  than  the  maximum  allowed  penetration,  because  if 
convergence  is  attained  with  penetrations  larger  than  this  value  this  contact  will  be 
released in subsequent steps and the simulation is likely destroyed.  Penetrations of this 
depth  are  likely  to  cause  discontinuities  along  line  searches  and  other  discouraging 
phenomena.  The user may of course scale the stiffness by increasing SFS but this also 
scales  the  stiffness  for  small  penetrations  and  probably  has  a  negative  effect  on 
convergence. 
Output for debugging 
Just as for implicit in general, Output is always a good thing to have when convergence 
starts  deteriorating  and  considering  the  release  of  contact  in  the  previous  section,  it 
would be interesting to know if penetrations are large enough for this to be a potential 
danger.  First, initial penetrations are always reported in the message file(s), including 
the  maximum  penetration  and  how  initial  penetrations  are  to  be  handled.    The  latter 
depends on the value of the IGNORE flag and this is dealt with Initial Penetrations.  In 
addition, by putting 
MINFO = 1 
on *CONTROL_OUTPUT, LS-DYNA will report the absolute maximum penetration as 
well  as  the  maximum  penetration  in  percentage  after  each  equilibrium.    If  the  relative 
maximum  penetration  reaches  above  99%  a  warning  message  is  printed  as  this 
particular contact is close to being released.  The output is exemplified in the following. 
Contact sliding interface          1 
Number of contact pairs          527 
Maximum penetration is  0.2447797E+00 between 
elements     306774 and     306672 
Maximum relative penetration is  0.2266694E+02 % between 
elements     306742 and     306733 
Contact sliding interface          2 
Number of contact pairs        16209 
Maximum penetration is   0.5027643E+00 between 
elements     219492 and      94935 
Maximum relative penetration is  1.0366694E+02 % between 
elements     219492 and      94935 
  *** Warning Penetration is close to maximum before release 
This  percentage  value  should  ideally  be  kept  below  some  90 %  to  have  some  sort  of 
comfort  margin.    There  are  three  ways  to  reduce  maximum  relative  penetrations,  and 
these are (i) to increase IGAP, (ii) to increase SST for solids or (iii) to increase SFS.  Note 
that  by  increasing  SST  for  solids  the  contact  stiffness  will  automatically  be  decreased,
APPENDIX P 
and this should be accompanied by increasing SFS by the square of the fraction increase 
of SST.  That is, if SST is doubled then SFS should be increased four times, and if SST is 
tripled then SFS should be increased nine times, and so on.  In this case even IGAP may 
have to be increased by some amount if being larger than unity in the first place. 
Initial Penetrations 
As  mentioned  above,  initial  penetrations  are  always  reported  in  the  message  file(s), 
including  the  maximum  penetration  and  how  initial  penetrations  are  to  be  handled.  
The IGNORE flag governs the latter and the options are 
IGNORE < 0 
IGNORE = 0 
IGNORE = 1 
IGNORE = 2 
IGNORE = 3 
IGNORE = 4 
Same functionality as the corresponding absolute value, but contact 
between segments belonging to the same part is ignored completely 
Initial  penetrations  will  give  rise  to  initial  contact  stresses,  i.e.,  the 
slave contact surface is not modified 
Initial  penetrations  will  be  tracked,  i.e.,  the  slave  contact  surface  is 
translated  to  the  level  of  the  initial  penetrations  and  subsequently 
follow the master contact surface on separation until the unmodified 
level is reached  
Initial  penetrations  will  be  ignored,  i.e.,  the  slave  contact  surface  is 
translated  to  the  level of  the  initial  penetrations,  optionally  with  an 
initial contact stress governed by MPAR1 
Initial penetrations will be removed over time, i.e., the slave contact 
surface  is  translated  to  the  level  of  the  initial  penetrations  and 
pushed  back  to  its  unmodified  level  over  a  time  determined    by 
MPAR1 
Same  as  IGNORE = 3  but  it  allows  for  large  penetrations  by  also 
setting MPAR2 to at least the maximum initial penetration 
The use of IGNORE depends on the problem, if no initial penetrations are present there 
is no need to use this parameter at all.  If penetrations are relatively small in relation to 
the  maximum  allowed  penetration,  then  IGNORE = 1  or  IGNORE = 2  seems  to  be  the 
appropriate choice.  For IGNORE = 2 the user may specify an initial contact stress small 
enough to not significantly affect the physics but large enough to eliminate rigid body 
modes  and  thus  singularities  in  the  stiffness  matrix.    The  intention  with  this  is  to 
constrain loose parts that are initially close but not in contact by pushing out the contact 
surface  using  SFST  and  applying  the  IGNORE = 2  option.    It  is  at  least  good  for 
debugging problems with many singular rigid body modes.  IGNORE = 3 is the Mortar 
interference counterpart, used for instance if there is a desire to fit a rubber component 
in a structure.  With this option the contact surfaces are restored linearly in time from 
the  beginning  of  the  simulation  to  the  time  specified  by  MPAR1.    A  drawback  with 
IGNORE = 3  is  that  initial  penetration  must  be  smaller  than  half  the  characteristic 
length of the contact or otherwise they will  not be detected in the  first place.   For this 
reason IGNORE = 4 was introduced where initial penetrations may be of arbitrary size, 
but  it  requires  that  the  user  provides  crude  information  on  the  level  of  penetration  of 
the contact interface.  This is done in MPAR2 which must be larger than the maximum
APPENDIX P 
penetration or otherwise and error termination will occur.  IGNORE = 4 only applies to 
solid elements at the moment. 
When eliminating penetrations by simulation for models with many parts, some parts 
may contain thin members that cause spurious self-contacts.  These may be difficult to 
work  around  by  only adjusting  contact  parameters,  but  fortunately  there  is  rarely  any 
loss of generality in ignoring contact within parts completely since those are usually not 
of interest in such a context.  The option IGNORE < 0 was implemented for this purpose 
and is a way to approach this problem. 
Damping 
Damping  can  be  activated  in  dynamic  implicit  analysis  using  VDC.    A  problem  with 
contact damping in implicit is that the time step is usually large enough to not resolve 
the time in contact to get the desired damping effect.  Often the situation becomes even 
worse, it is therefore not recommended to use damping. 
TROUBLESHOOTING CONVERGENCE PROBLEMS 
Convergence of the nonlinear equilibrium iteration process presents one of the greatest 
challenges  to  using  the  implicit  mode  of  LS-DYNA.    At  risk  of  repeating  what  has 
already been mentioned, below are some useful troubleshooting approaches. 
Eigenvalue Analysis 
Many  convergence  problems  in  static  implicit  analysis  are  caused  by  unconstrained 
rigid  body  modes.    These  are  created  when  an  insufficient  number  of  constraints  are 
applied to the model, or when individual model parts are left disconnected.  Eigenvalue 
analysis is an excellent diagnostic tool to check for these problems, both initially and at 
critical points in the simulation.  The procedure for performing an eigenvalue analysis 
was discussed Singularities and Eigenvalue Analysis. 
D3Iter Plot Database 
To  diagnose  convergence  trouble  which  develops  in  the  middle  of  a  simulation,  get  a 
picture of the deformed mesh.  Adjust the d3plot output interval to produce an output 
state  after  every  step  leading  up  to  the  problematic  time.    An  additional  binary  plot 
database  named  “d3iter”  is  available  which  shows  the  deformed  mesh  during  each 
equilibrium iteration.  This output is activated by 
D3ITCTL = 1 to activate d3iter plot database 
on *CONTROL_IMPLICIT_SOLUTION.  View this database using LS-PrePost to detect 
abnormal displacements.  The problem may become obvious, especially as deformation 
is magnified.  If not, there is yet another flag to activate to get the residual forces into 
both this database as well as d3plot for fringing.  Setting
APPENDIX P 
RESPLT = 1 to get residual data to binary databases 
on  *DATABASE_EXTENT_BINARY  will  do  just  that.    With  this  option  the  residual 
forces  are  output  to  the  d3plot  and  d3iter  databases  for  fringing  under  the  “NdV” 
menu.  This is a great tool for locating areas in the model where the residual forces are 
not being reduced to a satisfactory level and take appropriate actions. 
Taking Advantage of ASCII Information 
If  requested  through  Output  on  *CONTROL_IMPLICIT_SOLUTION  and  Output  for 
debugging  on  *CONTROL_OUTPUT,  a  lot  can  be  drawn  from  the  information  in  the 
message file(s).  This may be considered as a piece of advanced topic but may become 
useful in due time. 
Residual Norm 
Starting with the nonlinear output diagnostics, the following basic principle should be 
held  in  mind;  if  the  residual  norm  is  zero,  the  problem  is  solved.    So  it  all  comes  down  to 
make  this  number  (11)  small  enough  to  trust  the  results.    Therefore  we  suggest  to 
monitor the residual norm and interpret it as an indicator of whether the convergence 
characteristics  is  good.    Hopefully  you  would  see  this  number  decrease  with  implicit 
iterations and finally reach a relatively small number at convergence.  Although it may 
(and  will)  increase  on  occasion,  the  trend  should  be  a  decreasing  one.    If  this  is  a 
problem  from  the  get-go,  and  you  checked  the  model  integrity  through  Singularities 
and Eigenvalue Analysis and common practice, it may be that a feature is not properly 
supported in implicit. 
𝑒 
Line search not solvable 
Acceptable interval
𝑠 
𝑠 = 1
Smooth force, well 
behaved line search 
Discontinuous force, 
zero acceptable 
interval, indicates 
Line Search
APPENDIX P 
Another  thing  to  look  at  is  the  line  search  convergence  (9),  as  the  relatively  loose  line 
search  convergence  tolerance  should  render  a  reasonably  small  number  of  line  search 
iterations.  A rule of thumb would be less than 10, at most 20.  If more is used, or if the 
line search does not converge, there may be something in the model causing a jump in 
the residual forces.  This is not supposed to happen in implicit, and may suggest a bug.  
Either of the two following scenarios for a feature discontinuity (and many line search 
iterations) is possible 
•The line search step size becomes ridiculously small, and the current residual norm 
(7) is not approaching the initial one (3). 
•The  interval  in  which  the  optimal  step  is  to  be  found  (8)  becomes  ridiculously 
small,  and  the  residual  norm  on  the  left  and  right  interval  points  are  not  ap-
proaching  eachother.    This  situation  is  depicted  in  the  figure  above  (dashed 
line).  
Many line search iterations can of course be due to high nonlinearities but if the above 
is observed it should probably be investigated, for instance by trying to identify model 
features that may be causing the bad behavior.  If it is obvious that a discontinuity exist, 
like if the step size goes down to ~1−100 or the interval size becomes zero, and it is not 
due to a model error, please send a bug report. 
Stretching for Convergence 
If  the  problem  runs  fine  for  a  significant  number  of  load/time  steps  with  subsequent 
convergence  issues,  then  the  information  received  up  to  this  point  may  be  used 
intelligently  and  suggest  a  different  (unorthodox)  implicit  strategy.    To  justify  the 
approach,  we  begin  by  recalling  that  the  convergence  is  detected  by  the  following 
numbers  becoming  small;  𝑑 = ‖∆𝒖‖  (displacement  norm),  𝑟 = ‖𝑹‖  (residual  norm)  and 
𝑒 = ∣𝑹𝑇∆𝒖∣  (energy  norm).    But  all  these  numbers  are  linked  through  the  General, 
𝑲∆𝒖 = 𝑹, so if 𝑲 reasonably “nice” at all times it doesn’t matter which numbers we use 
for detecting convergence.  A mathematical way to state this is; if the condition number 
of 𝑲 is “good”, then all the norms are equivalent throughout the solution process.  An 
intuitive statement would be to say that the problem is only moderately nonlinear, and 
convergence  is  usually  never  a  problem.  But,  what  happens  if  the  properties  of  𝑲  are 
not that nice, or if 𝑲 shifts character every time it is reformed? This is sort of saying that 
the problem is highly nonlinear, for instance due to frequent change of contact state or 
onsets/offsets of plasticity.  In those cases the equivalence between 𝑑 and 𝑟 is lost, and 
typically  an  oscillatory  behavior  of  the  displacement  norm  is  observed  even  though  the 
residual norm is reducing, which in turn may lead to potential convergence problems just 
because the displacement criterion cannot be satisfied.  Or equally bad, it could lead to 
Premature Convergence just by the coincidence that the displacement norm happens to 
become small.  In those cases we essentially want to come up with a strategy where the 
displacement  criterion  is  taken  out  of  the  convergence  check  and  instead  detect 
convergence based on residual only.
So  assume  we  have  say  10  converged  states,  after  which  the  convergence  problems 
begin.  Then we can look at what the residual norm is for each of these converged states 
(11), for instance we may see the sequence  
APPENDIX P 
Step 1, residual norm 2859 
Step 2, residual norm 1581 
Step 3, residual norm 2119 
Step 4, residual norm 2511 
Step 5, residual norm 11570 
Step 6, residual norm 4904 
Step 7, residual norm 3586 
Step 8, residual norm 3157 
Step 9, residual norm 3315 
Step 10, residual norm 2825. 
For  each  of  these  steps  we  may  validate  the  results,  by  post-processing  contact  force 
curves,  checking  force/moment  balance  etc.,  in  LS-PrePost,  and  usually  there  is  a 
correlation  between  “good  results”  and  small  residual  norms.    Step  5  above  is  for 
instance  an  outlier  and  may  be  associated  with  a  prematurely  converged  step, 
something that can be confirmed or rejected from looking at the result.  The goal with 
these  observations  is  to  establish  a  reasonable  residual  norm  for  which  we  can  safely 
say that the results are good, and the numbers above indicates that 3000 may be a good 
candidate.    The  strategy  is  then  to  simply  put  DCTOL = 1.e-16  to  ignore  the 
displacement  and  set  ABSTOL = -3000,  which  means  we  can  be  assured  that 
convergence will not be detected until the residual norm is below 3000, and  we “know” 
from  having  learned  about  the problem  that  this  will  yield  good  results.    It  should  be 
mentioned  that  this  may  not  work  if  the  character  (force  level)  changes  significantly 
later on in the simulation, as 3000 then may not be the number we would trust. 
Contacts 
Continuing  with  the  Output  for  debugging,  a  general  rule  is  that  there  should  be  no 
warnings  of  large  penetrations  and  preferably  the  maximum  relative  penetration 
should be below  90%.  These numbers can be monitored after each load/time step.  If 
large penetrations occur, either increase IGAP or contact stiffness, whatever makes most 
sense,  but  first  make  sure  that  the  converged  step  is  really  converged  (no  Premature 
Convergence)  by  monitoring  the  residual  forces  and  checking  results  as  indicated 
above. 
CHECKLIST 
So, to summarize 
Activate implicit by setting IMFLAG = 1 on *CONTROL_IMPLICIT_GENERAL 
•Set DT0 to a reasonable initial time step
APPENDIX P 
Check possible singularities in an eigenvalue analysis by requesting NEIG 
eigenvalues on *CONTROL_IMPLICIT_EIGENVALUE 
•Find a way to constrain spurious modes 
Initially use dynamic analysis if rigid body modes are present in a static problem 
by setting IMASS = 1 on *CONTROL_IMPLICIT_DYNAMICS 
•Use TDYBIR, TDYDTH and TDYBUR 
•Use numerical damping by putting GAMMA = 0.6 and BETA = 0.38 
Only activate geometric stiffness contribution as a last resort, except for arc length 
methods 
Use default BFGS parameters ILIMIT and MAXREF on 
*CONTROL_IMPLICIT_SOLUTION  
•Increase or decrease ILIMIT based on convergence characteristics 
•Use full Newton (ILIMIT = 1) for hard problems 
•Keep MAXREF to a reasonably low number 
Use default convergence tolerances DCTOL, ECTOL and RCTOL on 
*CONTROL_IMPLICIT_SOLUTION 
•ABSTOL may be set to 1.e-20 to prevent premature convergence 
•Relaxing DCTOL may not necessarily result in better convergence 
•Future strategy may be to focus on residual 
Activate automatic time stepping on *CONTROL_IMPLICIT_AUTO 
•Set DTMAX to a number that resolves features of interest 
Contacts 
Material nonlinearities 
Frequencies 
Use default line search method on *CONTROL_IMPLICIT_SOLUTION 
•Switch to LSMTD = 5 if hard problem (typically rubbers) 
•Don’t change LSTOL 
Use at least NLPRINT = 2 on *CONTROL_IMPLICIT_SOLUTION to get conver-
gence diagnostics into log files 
•Use NLPRINT = 3 to thoroughly track the residual norm and monitor line 
search behavior if debugging model is necessary 
Use *CONTROL_IMPLICIT_SOLVER only in special occasions 
Set D3ITCTL = 1 on *CONTROL_IMPLICIT_SOLUTION to get a database with 
Newton iterates when debugging a model 
•Complement this with RESPLOT = 1 on *DATABASE_EXTENT_BINARY to 
get the possibility to fringe the residual force vector 
For forming Mortar contact, make sure 
•Tools are oriented towards the blank
APPENDIX P 
•Contact on top and bottom of blank are separated among contact interfaces 
Use part (set) definitions of slave and master in Mortar contact 
Always use weak part as slave in a Mortar contact definition to get best possible 
convergence 
Set SST to a reasonable characteristic length for slave side consisting of solid 
elements 
•With this option, separate solids and shells into different contact interfaces 
in order to not manipulate the contact thickness for shells 
 If penetrations are large, activate penetration diagnostics on 
*CONTROL_CONTACT 
To avoid release of contact pairs, either 
•Increase stiffness scaling factor SFS 
•Increase IGAP for progressive stiffness increase 
•Increase SST for solids while at the same time increasing SFS 
Use IGNORE appropriately to deal with initial penetrations 
•Check initial penetrations in message file 
Don’t use contact damping
APPENDIX Q 
APPENDIX Q:  User Defined Weld Failure 
The  addition  of  a  user  weld  failure  subroutine  into  LS-DYNA  is  relatively  simple.    The 
UWELDFAIL  subroutine  is  called  every  time  step  when  OPT = 2  is  specified  in  MAT_-
SPOTWELD.   As data, the identification number for the spotweld material, six constants 
specified in the input by thfe locations NRR through MTT, the radius of the cross section 
of  the  spotwelds,  the  current  time,  and  the  current  values  of  the  resultants  for  the 
spotwelds, which are stored in array STRR, are passed to the subroutine.  The subroutine 
loops over the welds from LFT through LLT, and sets the values of the failure flag array 
FLAG. 
      SUBROUTINE UWELDFAIL(IDWELD,STRR,FAIL,FIBL,CM,TT,LFT,LLT) 
C****************************************************************** 
C|  LIVERMORE SOFTWARE TECHNOLOGY CORPORATION  (LSTC)             | 
C|  ------------------------------------------------------------  | 
C|  COPYRIGHT 2002 JOHN O.  HALLQUIST, LSTC                        | 
C|  ALL RIGHTS RESERVED                                           | 
C****************************************************************** 
C 
C***  SPOTWELD FAILURE ROUTINE 
C 
C***  LOCAL COORDINATES: X IS TANGENT TO BEAM, Y & Z ARE NORMAL 
C 
C***  VARIABLES 
C          IDWELD ---- WELD ID NUMBER 
C          STRR ------ STRESS RESULTANTS 
C                      (1) AXIAL (X DIRECTION) FORCE 
C                      (2) Y SHEAR FORCE 
C                      (3) Z SHEAR FORCE 
C                      (4) MOMENT ABOUT Z 
C                      (5) MOMENT ABOUT Y 
C                      (6) TORSIONAL RESULTANT 
C          FAIL ------ FAILURE FLAG 
C                      = 0 NOT FAILED 
C                      = 1 FAIL ELEMENT 
C          FIBL ------ LOCATION (1,*) GIVES THE SPOTWELD DIAMETER 
C          CM -------- 6 CONSTANTS SUPPLIED BY USER 
C          TT -------- CURRENT SIMULATION TIME 
C          LFT,LLT --- DO-LOOP RANGE FOR STRR 
C 
      DIMENSION IDWELD(*),STRR(6,*),FAIL(*),CM(*),FIBL(5,*) 
C           
C 
      RETURN 
      END
APPENDIX R 
APPENDIX R:  User Defined 
Cohesive Model 
The addition of a user cohesive material subroutine into LS-DYNA is relatively simple.  
The UMATiC subroutine is called every time step where i ranges from 41 to 50.   Input 
for the material model follows the *MAT_USER_DEFINED_MATERIAL definition.  The 
user has the option of providing either a scalar or vectorized subroutine.  As discussed 
in  the  Remarks  for  the  user-defined  material,  the  first  two  material  parameters  are 
reserved  to  specify  how  the  density  is  treated  and  the  number  of  integration  points 
required for the failure of the element. 
The  cohesive  model  calculates  the  tractions  on  the  mid-surface  of  the  element  as  a 
function of the differences of the displacements and velocities of the upper (defined by 
nodes  5-6-7-8)  and  lower  surfaces  (defined  by  nodes  1-2-3-4).    The  displacements, 
velocities, and the calculated tractions are in the local coordinate system of the element, 
where the first two components of the vectors are in the plane of the mid-surface and 
the third component is normal to the mid-surface. 
A  stiffness  must  also  be  calculated  by  the  user  for  the  explicit  time  step  calculation  in 
LS-DYNA.    This  stiffness  must  provide  an  upper  bound  on  the  stiffness  in  all  three 
directions. 
The  material  fails  at  an  integration  point  when  ifail=.true.    For  an  element  to  be 
deleted  from the  calculation,  the  number  of  integration  points  specified  by  the  second 
material  parameter  must  fail.    If  the  second  parameter  is  zero,  elements  cannot  fail 
regardless of the specification of IFAIL in the user-defined material input.  For example, 
the user may choose to reject an implicit step is the displacement increment is too 
For  implicit  analysis,  the  subroutine  is  called  with  maketan=.true.  and  the  user  must 
provide the elastic moduli in the three local directions in the respective diagonal terms 
of the dsave array.  The parameter reject, if set to .true. by the user, will signal to LS-
DYNA  that  the  current  implicit  iteration  is  unacceptable.    For  example,  the  user  may 
choose to reject an implicit step if the traction changes too much from the last time step.  
In  this  situation,  LS-DYNA  will  print  a  warning  message  `Material  model  rejected 
current iterate’ and retry the step with a smaller time step.  If chosen carefully (by way 
of  experimenting),  this  may  result  in  a  good  trade-off  between  the  number  of  implicit 
iterations per step and the step size for overall speed. 
The following example is a vectorized model with two elastic constants and failure: 
      subroutine umat41c(idpart,cm,lft,llt,fc,dx,dxdt,aux,ek, 
     & ifail,dt1siz,crv,nnpcrv,nhxbwp,cma,maketan,dsave,ctmp,elsiz, 
     & reject,ip,nip) 
      include 'nlqparm'
APPENDIX R 
c***  vector cohesive material user model example 
c 
c***  variables 
c          idpart ---- Part ID 
c          cm -------- material constants 
c          lft,llt --- start and end of block 
c          fc -------- components of the cohesive force 
c          dx -------- components of the displacement 
c          dxdt ------ components of the velocity 
c          aux ------- history storage 
c          ek -------- max.  stiffness/area for time step calculation 
c          ifail ----- =.false.  not failed 
c                      =.true.  failed 
c          dt1siz ---- time step size 
c          crv ------- curve array 
c          nnpcrv ---- # points per curve for crv array 
c          nhxbwp ---- internal element id array, lqfinv(nhxbwp(i),2) 
c                      gives external element id 
c          cma ------- additional memory for material data defined by  
c                      LMCA in 2nd card, 6th field of *MAT_USER_DEFINED 
c          maketan --- true for implicit 
c          dsave ----- material stiffness array, define for implicit 
c          ctmp ------ current temperature  
c          elsiz ----- characteristic element size (=sqrt(area)) 
c          reject ---- set to .true.  if this implicit iterate is 
c                      to be rejected for some reason (implicit only) 
c          ip -------- integration point number 
c          nip ------- total number of integration points 
c 
c***  dx, dxdt, and fc are in the local coordinate system: 
c     components 1 and 2 are in the plane of the cohesive surface 
c     component 3 is normal to the plane 
c 
c***  cm storage convention 
c     (1) =0 density is per area 
c         =1 density is per volume 
c     (2) number of integration points for element deletion 
c         =0 no deletion 
c     (3:48) material model constants 
c 
      logical ifail,maketan,reject 
      dimension cm(*),fc(nlq,*),dx(nlq,*),dxdt(nlq,*), 
     &          aux(nlq,*),ek(*),ifail(*),dt1siz(*),crv(101,2,*), 
     &          nhxbwp(*),cma(*),dsave(nlq,6,*),ctmp(*),elsiz(*) 
      integer nnpcrv(*) 
c 
c 
      et=cm(3) 
      en=cm(4) 
      eki=max(et,en) 
      fcfail=cm(5) 
c 
      do i=lft,llt 
        fc(i,1)=et*dx(i,1) 
        fc(i,2)=et*dx(i,2) 
        fc(i,3)=en*dx(i,3) 
        ek(i)=eki 
        ifail(i)=fc(i,3).gt.fcfail 
      enddo 
c 
      if(maketan) then 
        do i=lft,llt 
          dsave(i,1,1)=et 
          dsave(i,2,1)=0. 
          dsave(i,3,1)=0. 
          dsave(i,1,2)=0.
APPENDIX R 
          dsave(i,2,2)=et 
          dsave(i,3,2)=0. 
          dsave(i,1,3)=0. 
          dsave(i,2,3)=0. 
          dsave(i,3,3)=en 
        enddo 
      endif 
      return 
      end 
The  second  example  implements  the  Tveergard-Hutchinson  cohesive  model  with 
failure in both the vectorized (UMAT42C) and scalar (UMAT43C) forms.  Note the LFT 
and LLT are passed to the scalar version, however their value is zero. 
      subroutine umat42c(idpart,params,lft,llt,fTraction,jump_u,dxdt, 
     & aux,ek,ifail,dt1siz,crv,nnpcrv,nhxbwp,cma,maketan,dsave,ctmp,elsiz, 
     & reject,ip,nip) 
      include 'nlqparm' 
c 
c***  vector cohesive material user model example 
c 
c     Tveergard-Hutchinson model based on: 
c     tahoe/src/elements/cohesive_surface/cohesive_models/TvergHutch3DT.cpp 
c 
c     the declaration below is processed by the C preprocessor and 
c     is real*4 or real*8 depending on whether LS-DYNA is single or double 
c     precision 
c 
      REAL L,jump_u 
      logical ifail,maketan,reject 
      dimension params(*),fTraction(nlq,*),jump_u(nlq,*),dxdt(nlq,*), 
     &          aux(nlq,*),ek(*),ifail(*),dt1siz(*),crv(101,2,*), 
     &          nhxbwp(*),cma(*),dsave(nlq,6,*),ctmp(*),elsiz(*) 
      integer nnpcrv(*) 
c 
      fsigma_max=params(3) 
      fd_c_n=params(4) 
      fd_c_t=params(5) 
      fL_1=params(6) 
      fL_2=params(7) 
      fpenalty=params(8) 
c 
      fK=fpenalty*fsigma_max/(fL_1*fd_c_n) 
c 
      fac=min(fd_c_n/fd_c_t**2,1./fd_c_n) 
c 
      do i=lft,llt 
      u_t1 = jump_u(i,1) 
      u_t2 = jump_u(i,2) 
      u_n = jump_u(i,3) 
c 
      r_t1 = u_t1/fd_c_t 
      r_t2 = u_t2/fd_c_t 
      r_n = u_n/fd_c_n 
      L = sqrt(r_t1*r_t1 + r_t2*r_t2 + r_n*r_n) 
c  
      if (L .lt.  fL_1) then 
         sigbyL=fsigma_max/fL_1
APPENDIX R 
      else if (L .lt.  fL_2) then 
         sigbyL = fsigma_max/L 
      else if (L .lt.  1.) then 
         sigbyL = fsigma_max*(1.  - L)/(1.  - fL_2)/L 
      else 
         sigbyL = 0.0    
         ifail(i)=.true. 
      endif 
c  
      fTraction(i,1) = sigbyL*r_t1*(fd_c_n/fd_c_t) 
      fTraction(i,2) = sigbyL*r_t2*(fd_c_n/fd_c_t) 
      fTraction(i,3) = sigbyL*r_n 
c 
c     penetration  
      if (u_n .lt.  0) fTraction(i,3)=fTraction(i,3)+fK*u_n 
c 
c     approximate stiffness for time step 
      if (u_n .lt.  0) then 
        ek(i)=fac*sigbyL+fK  
      else 
        ek(i)=fac*sigbyL 
      endif 
c 
      if (maketan) then 
        dsave(i,1,1)=sigbyL/fd_c_t*(fd_c_n/fd_c_t) 
        dsave(i,2,1)=0. 
        dsave(i,3,1)=0. 
        dsave(i,1,2)=0. 
        dsave(i,2,2)=sigbyL/fd_c_t*(fd_c_n/fd_c_t) 
        dsave(i,3,2)=0. 
        dsave(i,1,3)=0. 
        dsave(i,2,3)=0. 
        dsave(i,3,3)=sigbyL/fd_c_n 
        if (u_n.lt.0) dsave(i,3,3)=dsave(i,3,3)+fk 
      endif 
      enddo 
c 
      return 
      end 
c 
c 
c       
      subroutine umat43c(idpart,params,lft,llt,fTraction,jump_u,dxdt, 
     & aux,ek,ifail,dt1siz,crv,nnpcrv,nhxbwp,cma,maketan,dsave,ctmp,elsiz, 
     & reject,ip,nip) 
c 
c***  scalar cohesive material user model example 
c 
c     Tveergard-Hutchinson model based on: 
c     tahoe/src/elements/cohesive_surface/cohesive_models/TvergHutch3DT.cpp 
c 
c     the declaration below is processed by the C preprocessor and 
c     is real*4 or real*8 depending on whether LS-DYNA is single or double 
c     precision 
c 
      REAL L,jump_u 
      logical ifail,maketan,reject 
      dimension params(*),fTraction(nlq,*),jump_u(nlq,*),dxdt(nlq,*), 
     &          aux(nlq,*),ek(*),ifail(*),dt1siz(*),crv(101,2,*), 
     &          nhxbwp(*),cma(*),dsave(nlq,6,*),ctmp(*),elsiz(*) 
      integer nnpcrv(*) 
c 
      fsigma_max=params(3) 
      fd_c_n=params(4) 
      fd_c_t=params(5) 
      fL_1=params(6)
APPENDIX R 
      fL_2=params(7) 
      fpenalty=params(8)  
c 
      fK=fpenalty*fsigma_max/(fL_1*fd_c_n) 
c 
      fac=min(fd_c_n/fd_c_t**2,1./fd_c_n) 
c  
      u_t1 = jump_u(1) 
      u_t2 = jump_u(2) 
      u_n = jump_u(3) 
c      
      r_t1 = u_t1/fd_c_t 
      r_t2 = u_t2/fd_c_t 
      r_n = u_n/fd_c_n 
      L = sqrt(r_t1*r_t1 + r_t2*r_t2 + r_n*r_n)  
c  
      if (L .lt.  fL_1) then 
         sigbyL=fsigma_max/fL_1 
      else if (L .lt.  fL_2) then 
         sigbyL = fsigma_max/L 
      else if (L .lt.  1.) then 
         sigbyL = fsigma_max*(1.  - L)/(1.  - fL_2)/L 
      else 
         sigbyL = 0.0    
      ifail=.true. 
      endif 
c  
      fTraction(1) = sigbyL*r_t1*(fd_c_n/fd_c_t) 
      fTraction(2) = sigbyL*r_t2*(fd_c_n/fd_c_t) 
      fTraction(3) = sigbyL*r_n 
c  
c     penetration  
      if (u_n .lt.  0) fTraction(3)=fTraction(3)+fK*u_n 
c  
c     approximate stiffness for time step 
      if (u_n .lt.  0) then 
        ek=fac*sigbyL+fK  
      else 
        ek=fac*sigbyL 
      endif 
c 
      if (maketan) then 
        dsave(1,1)=sigbyL/fd_c_t*(fd_c_n/fd_c_t) 
        dsave(2,1)=0. 
        dsave(3,1)=0. 
        dsave(1,2)=0. 
        dsave(2,2)=sigbyL/fd_c_t*(fd_c_n/fd_c_t) 
        dsave(3,2)=0. 
        dsave(1,3)=0. 
        dsave(2,3)=0. 
        dsave(3,3)=sigbyL/fd_c_n 
        if (u_n.lt.0) dsave(3,3)=dsave(3,3)+fk 
      endif 
      return 
      end
APPENDIX S 
APPENDIX S:  User Defined 
Boundary Flux 
A user defined boundary flux interface is provided in LS-DYNA where it is possible to 
define the thermal heat flux (power per surface area) in or out of a surface segment as 
an  arbitrary  function  of  temperature  and  history.    The  user  may  associate  history 
variables with each individual flux interface and also use load curves. 
The  user  flux  interface  is  invoked  using  the  keyword  *BOUNDARY_FLUX_OPTION.  
This  is  accomplished  with  the  parameter  NHISV.    When  it  is  defined  with  a  value 
greater than 0, the user subroutine 
subroutine usrflux(fl,flp,…) 
is  called  to  compute  the  flux  (fl)  defined  as  heat  (energy)  per  time  and  per  surface 
area.  
Other parameters that are passed to the user flux subroutine include the segment nodal 
temperatures at the previous (T0) and current time (T1), the segment nodal coordinates 
and the time integration parameter α.  Also, the current thermal simulation time t, the 
time step Δt and average segment temperature (Tα) at time t+αΔt is provided together 
with  the  curve  array  for  accessing  defined  load  curves  in  the  keyword  input  file.    For 
computing  load  curve  values,  note  that  load  curve  IDs  need  to  be  transformed  to 
internal  numbers  or  the  subroutine  crvval  should  be  used,  see  the  appendix  on  user 
defined materials for details.  
The segment coordinates available in the subroutine are such that the outward normal 
vector  follows  the  well-known  right-hand  rule,  thus  segments  corresponding  to  the 
lower surface of thick thermal shells are reversed before passed to the subroutine.  For 
shells in general, the segment connectivity should follow the connectivity of the actual 
shell element to avoid problems. 
Optionally, the user may define the derivative of the flux fl with respect to the average 
segment  temperature  (Tα)  at  time  t+αΔt,  flp.    This  value  is  used  in  the  nonlinear 
thermal solver for assembling the correct stiffness matrix and must be set by the user.  If 
possible,  it  is  recommended  to  use  a  value  that  reflects  the  nonlinearity  of  the  flux 
model, otherwise the value 0 should be used. 
An  array  of  history  variables,  identical  with  the  input  parameters  defined  in  the 
keyword input file, are passed to the subroutine that can be updated with time or kept 
constant  throughout  the  simulation.    An  example  of  usage  would  be  to  integrate  the 
flux  with  time  to  keep  track  of  the  dissipated  energy  per  surface  area  in  order  to 
simulate the effects of spray cooling in hot-stamping.
APPENDIX S 
time) 
(input) 
      subroutine usrflux(fl,flp,x,tnpl,tnl,nodes, 
     .     alpha,atime,atemp,dt,time,fhsv,nfhsv,crv) 
C****************************************************************** 
C|  LIVERMORE SOFTWARE TECHNOLOGY CORPORATION  (LSTC)             | 
C|  ------------------------------------------------------------  | 
C|  COPYRIGHT © 2007 JOHN O.  HALLQUIST, LSTC                      | 
C|  ALL RIGHTS RESERVED                                           | 
C****************************************************************** 
c      
c     User subroutine for boundary thermal flux 
c 
c     Purpose:  To define thermal flux parameter (heat per surface area and 
c 
c      
c     Variables: 
c 
c     fl              = flux intensity (output)                 
c     flp             = flux intensity derivative wrt atemp (output) 
c     x(3,nodes)      = global segment coordinates (input)         
c     tnpl(nodes)     = temperatures at time time (input)           
c     tnl(nodes)      = temperatures at time time-dt (input) 
c     nodes           = number of nodes in segment (3,4 or 6) (input) 
c     alpha           = time integration parameter (input)       
c     atime           = time+(alpha-1)*dt 
c     atemp           = average segment temperature at time atime 
c     dt              = time step size (input)                                
c     time            = time at which the new temperature is sought (input) 
c     fhsv(nfhsv)     = flux history variables (input/output) 
c     nfhsv           = number of flux history variables for this segment 
c 
c     crv             = curve array (input) 
c 
      include 'nlqparm' 
      dimension x(3,*),tnpl(*),tnl(*) 
      dimension fhsv(*),crv(lq1,2,*) 
c 
c     Define flux by linear convection 
c     that optionally decays (in an ad-hoc way) as power  
c     dissipates from surface 
c      
c     fhsv(1) = convection coefficient 
c     fhsv(2) = ambient temperature 
c     fhsv(3) = total amount of energy per surface area available 
c     fhsv(4) = dissipated energy per surface area at current 
c      
      hcon=fhsv(1) 
      tinf=fhsv(2) 
      flin=hcon*(tinf-atemp) 
      if (nfhsv.gt.2) then 
         q=(1.-fhsv(4)/fhsv(3))/ 
     .        (1.+.5*dt*flin/fhsv(3)) 
         flp=-q*hcon 
         if (q.gt.1.) then 
            q=1. 
            flp=-hcon 
         elseif (q.lt.0.) then 
            q=0. 
            flp=0. 
         endif          
         fl=q*flin         
         fhsv(4)=fhsv(4)+dt*.5*fl 
         fhsv(4)=min(fhsv(3),fhsv(4)) 
      else 
         fl=flin 
         flp=-hcon 
      endif
APPENDIX S 
c      
      return 
      end
APPENDIX T:  Metal Forming Glossary 
A TYPICAL DRAW DIE ENGINEERING PROCESS 
Clay models of a new vehicle are scanned and the outer shell surfaces are created in a 
design studio.  Body-in-white engineers and designers are responsible to create all the 
inner  parts  and  various  structure  and  underbody  parts.    Flanges  are  created  on  outer 
surface parts to be joined with the inner panels.  These parts are typically created in the 
car  axis;  with  global  X-axis  runs  from  the  front  to  the  back  along the  car’s  center  line, 
global Y-axis from the driver side to the passenger side and Z-axis going straight up. 
During  the  clay  design  and  shaping,  simultaneous  and  multidisciplinary  engineering 
may  be  practiced  involving  divisions/departments  from  design,  engineering  and 
manufacturing.  Material suppliers may also be involved in this stage for consultation if 
advanced materials are to be applied.  Multidisciplinary involvement in this early stage 
of a vehicle development allows manufacturing engineers to capture any part designs 
with  “no  make”  conditions  that  would  be  costly  if  they  were  allowed  to  proceed  to  a 
later  stage;  while  design  envelopes  can  be  pushed  to  their  maximum  potential  within 
the state-of-art manufacturing capabilities. 
During  the  advance  feasibility  phase,  parts  from  the  design  studio  are  processed 
quickly  to  go  through  an  engineering  process  involving  mainly  the  process  engineer 
and  FEA  simulation  engineer.    Addendum  and  binder  are  roughly  built  in  order  to 
conduct a reliable draw die simulation.  The exact process eventually would be used to 
build  the  die  may  not  yet  be  established,  therefore  similar  processes  from  knowledge 
base  are  used  as  references.    Rarely  are  secondary  dies  (all  dies  except  draw  die) 
simulated.    The  main  task  here  is  to  provide  some  quick  assessment  of  the  part’s 
manufacturability through fast design/engineering iterations. 
During the hard die design and construction phase, stamping manufacturing processes 
(some  in  three  dimensional)  are  established,  by  referring  to  existing  knowledge  base, 
with necessary modifications needed for the current part design, and with the limits of 
manufacturing  equipment  such  as  press  type,  shut  height,  maximum  tonnage  and 
automation,  etc.    The  stamping  process  includes  the  number  of  dies  (to  make  a 
complete part of the final shape), part tipping, draw height, trimming (direct or aerial), 
flanging, springback compensation requirements, etc.  Not all areas of the part may be 
formed to its final shape in one draw die.  Some involve redraw die if one area of the 
part  is  especially  deep  compared  to  the  rest  of  the  part,  which  may  otherwise  cause 
uncontrollable wrinkles, splits, or exceed the draw height limit without the redrawing.  
Some areas of the part (which may have “undercut” or “die locked” conditions) may be 
unfolded to the addendum, then trimmed and flanged in a flanging die later.  A typical
APPENDIX T 
example  of  such  can  be  found  along  the  hood  line  of  a  fender  outer.    There  may  be 
multiple  trimming  and  flanging  dies,  since  not  all  areas  of  the  drawn  panel  may  be 
feasible for trimming or flanging all in one trim or flanging die. 
Referring to Figure 63-1, a typical draw die development process flow for an outer part 
is  illustrated.    The  part  is  tipped  from  the  global  car  axis  to  a  ‘draw  die’  axis,  which 
takes  into  account  of  balancing  the  internal  draw  angles  over  the  entire  part,  and 
minimizing  the  overall  draw  height,  etc.    Hem  flanges  are  unfolded  off  the  part 
breakline (Figure 63-1) in one of the following ways: 
1)Tangent extension of the part surface, 
2)Horizontal surface, 
3)Vertical down-standing surface, 
4)Any angled surface between horizontal and vertical surface, 
5)To the addendum surfaces to be designed; in this case, the unfolding will happen 
after the addendum design is complete. 
Flange  unfold  must  take  into  account  the  trimming  condition  later  in  the  trim  dies.  
Direct  trim  represents  the  trim  steel  going  down  in  a  draw  direction  (vertical);  while 
aerial  (cam)  trim  steel  covers  all  other  directions,  driven  by  a  ‘cam  driver’  driven 
further by the vertical downward motion of the trim die.  There are specific trim angle 
requirements  for  direct  and  aerial  trim  operations.    Next,  the  part  boundary  is 
smoothed, filling up any gaps, holes and sharp features.  The boundary will likely be 
modified later during the addendum build.  Binder is created, based on the unfolded 
part  boundary  and  overall  part  curvature.    A  developable  binder  surface,  which 
consists of planes, cylindrical surfaces or a combination of both, is preferred; however, 
in  some  cases  a  doubly  curved  binder  surface  (undevelopable  surface)  must  be 
designed for the purpose of reducing the  draw depth at  critical locations for material 
utilization,  alleviating  thinning,  or  both.    Theoretical  punch  opening  line  (P.O.    line, 
Detail  #2  in  Figure  63-1)  can  be  offset  from  the  smoothed  part  boundary  in  the  plane 
normal  to  the  draw  axis,  projected  to  the  binder  surface  in  the  draw  direction;  some 
smoothing of the P.O.  lines may be required.  Generally, the finished P.O.  lines should 
be consisted of mostly straight lines and radii, with generous transition among corners.  
P.O.  lines do not follow tight corners, avoiding formation of wrinkles during the draw.  
In  addition,  design  of P.O.    lines  must  take  into  consideration the material  utilization 
issue,  especially  in  the  blank  sizing  critical  locations.    Once  P.O.    lines  design  is 
complete,  binder  surfaces  inside  of  the  P.O.    are  trimmed  and  the  remaining  binder 
surface  design  is  sent  for  binder  closing  simulation.    Given  a  blank  initial  shape, 
simulation of the binder closing action can determine the quality of the binder design.  
Typically,  for  exterior  outer  panels,  no  buckles  or  wrinkles  are  allowed  during  the 
closing;  for  inner  panels,  some  wrinkles  are  acceptable,  or  even  desirable,  depending 
on the part shape.  Lower punch/post support may be introduced to reduce the draw 
height,  alleviate  thinning,  or  remove  the  initial  blank  drape  into  the  binder  cavity.  
Based on the binder closing simulation results, unacceptable binder design is sent back 
for rework, and the satisfactory binder design proceeds into the next step of addendum
APPENDIX T 
build, which is used to fill the space between the part boundary and binder surface.  It 
is noted that the P.O.  lines may need to be adjusted during the addendum design.  The 
trimming condition may also be affected and modified  during the addendum design.  
Next, draw simulation ensues, assessing the overall formablity of the draw design.  If 
quality targets are not achieved in the simulation, the process may go all the way back 
to  the  tipping  for  redesign/reprocess;  otherwise  successful  simulation  will  direct  the 
draw surface design to the next stage of draw die structure design. 
TYPES OF DRAW DIES 
There  are  many  different  types  of  draw  dies  used  to  punch  the  part  to  their  intended 
shape, as shown in Figure 63-2.  They basically can be divided into either single action 
or double action dies.  Specifically (names may vary among different companies), 
1)Air draw ― Single action. It is a 3-piece die system with 1 piece upper (cavity) and 
2-piece  (binder  and  punch/post)  lowers.    The  upper  cavity  (driven  by  press 
ram) moves down in one action to close with the lower binder, and then closes 
with the lower punch to draw the part to the home position.  The lower binder is 
either  sitting  on  an  air  cushion  through  pins  that  go  through  the  press  bed,  or 
directly  on  nitrogen  cylinders  arranged  uniformly  between  the  bottom  of  the 
binder structure and the press bed; the punch is fixed onto the press bed.  This is 
the  most  popular  draw  type,  mainly  because  of  its  speed  and  efficiency.    Its 
limitation includes a maximum draw height of 10”. 
2)Toggle draw ― Double action. It is a 3-piece die system with 2-piece upper (binder 
and punch) and 1 piece (cavity) lower.  Upper binder, driven by the outer ram of 
the press, moves down to clamp the blank with the lower cavity; then the upper 
punch, driven down by the inner ram, closes with the lower cavity to complete 
the draw.  Since this adds another action, it is slower than the air draw; howev-
er, this type of draw die is well suited to control the wrinkles created during the 
forming of difficult part, such as liftgate and door inner.  Furthermore, this type 
of draw has a relatively large draw height, which is limited only by the press. 
3)Air  draw  with  pressure  pad  ―  Single  action.  This  is  very  similar  to  1),  except  an 
additional pressure pad, driven by nitrogen cylinders mounted on the upper die 
structure, closes first  with the lower punch, then the entire upper comes down 
to finish the draw.  This is similar to 1) in efficiency. 
4)Stretch Draw (four piece) ― Double action.  It is a 4-piece die system with 2-piece 
uppers (upper binder and punch) and 2-piece lowers (lower binder and cavity).  
Upper  binder  moves  down  to  close  with  lower  binder,  moving  together  for  a 
certain  distance  (up  to  2”),  then  upper  punch  comes  down  to  completely  close 
with lower cavity.  Finally the binders move down together to their home posi-
tion.  This process is not used as often as 1), 2) and 3), however, it is very capable 
in  forming  difficult  inner  parts,  especially  those  prone  for  wrinkles,  such  as 
liftgate inner, door inner and floor pan.  Since there is a ‘pre-stretch’ action with
APPENDIX T 
the binders clamping the blank and moving down together, strain path change 
in the part during the forming is expected.  This is the slowest draw type. 
5)Crash  Form  Die  ―  Single  action.    It  is  a  2-piece  die  system  with  no  upper  or 
binders.  Upper and lower tool takes the same shape, with upper moving down 
to  close  with  the  lower  tool.    This  is  obviously  a  very  simple  die,  which  can 
handle  simple  parts,  with  not  too  much  draw  depth  variation  (near  constant 
draw depth all around). 
TYPES OF FLANGING DIES 
There are three types of flanging dies, as shown in Figure 63-3.  All three types have a 
fixed lower (trim) post upon which the drawn (or partially trimmed part) is sitting, and 
a pressure pad (or multiple pads) which holds the part (which is loaded onto the post in 
a vertical direction) in place against the post.  In a direct flanging process, the flanging 
steel  (Figure  63-3)  moves  vertically  down  to  ‘wipe’  or  ‘bend’  the  part  to  its  flanged 
position.  In an aerial flanging process, the flanging steel moves to form the flanges in 
an angle rather than the vertical direction.  The steel is held by the cam slide, driven by 
a cam driver which in turn is driven by the trim die’s downward movement.  Since the 
finished flange forms a ‘die lock’ condition, meaning the flanged part will not be able to 
be lifted (retract) out of the trim die into the next die (or station), the filler cam (Figure ) 
is moved horizontally out of the way so the part can be lifted up and out.  Once the part 
is removed, the filler cam moves back into its home position ready for the next drawn 
panel to be loaded.  In the rotary cam flanging process, the filler cam is called a ‘rotor’, 
which rotates out of the way for the flanged part to be lifted up and out.  Some parts of 
the  rotary  cam  flanging  design  are  a  patented  process.    In  comparison  to  the 
conventional cam flanging, rotary flanging has the advantage of being very compact. 
TYPES OF HEMMING DIES 
There are two types of hemming dies, as shown in Figure 63-4.  Both processes have a 
fixed hemming bed, on which the flanged outer part is loaded; the inner panel is then 
loaded onto the outer panel; proper clamps are applied to hold tight the panels together 
and in place.  In press (or table top) hemming, a pre-hemming tool is moved to form the 
flange  into  a  halfway  position,  followed  by  the  final  hemming  tool  pressing  down  on 
the flange against the inner and outer panels to its final position.  Many different shapes 
of  hem  tips  can  be  achieved,  as  shown  in  the  figure.    In  roller  hemming,  a  pre-roller 
moves in a three dimensional curvilinear path following the hem tip, to form the flange 
partially.  This is followed by a final roller, moving in another three dimensional path, 
to  finish  the  hem  shape.    In  the  hemming  of  complex  or  high-end  parts,  many  passes 
(rollers) are needed to achieve high quality hem surfaces.  Similarly, with the design of 
different roller shapes, many shapes of hem tips can be achieved.
APPENDIX T
APPENDIX T 
Body-in-white part
Tipping
Unfold hem/flanges
Detail #1
Detail #2
Unfolded part 
boundary
Smoothed 
boundary
P.O./Binder design
Not OK
OK
Binder closing 
simulation
Fill/smoothing of part 
boundary (3-D)
Detail #2
Draw 
simulation
Not OK
OK
Die structure 
design
Addendum design/P.O. adjust
Trim line
Part/Product
Scrap
Unfold hem flange 
tangentially 
Hem flange 
or, unfold to 
flanging position 
Detail #1
Break line
Punch opening line
(Theoretical P.O. line, 
vertical project to the 
binder surface) 
Draw wall surface
Post(punch) radius
Draw wall angle
Die radius
Binder surface
Detail #2
Figure 63-1.  A typical draw die engineering process
APPENDIX T 
1 2
Air draw+
Toggle draw+ Air draw with pad
Four-piece
 stretch draw++ Crash form die+
+ :      single action
++ :  double action
Figure 63-2.  Types of draw dies 
Pad
Sheet blank
Post
Flanging steel
Pad 1
Sheet blank (initial)
Post
Filler cam
Cam steel
Cam slide
Sheet blank (final)
Direct flanging
Cam (aerial) flanging
Pad 1
Post
Rotor
Sheet blank (initial)
Cam steel
Cam slide
Sheet blank (final)
Rotary cam flanging
Figure 63-3.  Types of flanging dies
APPENDIX T 
Final hemming  tool
3D curlverlinear roller 
path along hem flange
Inner panel
Clamper
Straight motions
Final roller
Pre-hemming  tool
Detail #3
Outer panel
Hem bed
Hem bed
Pre-roller
Press (or table top) hemming
Roller hemming
Inner panel
Outer panel
Detail #3 (loop hem)
Figure 63-4.  Types of hemming dies
APPENDIX P

Corporate Address 
Livermore Software Technology Corporation 
P. O. Box 712 
Livermore, California 94551-0712 
Support Addresses 
Livermore Software Technology Corporation 
7374 Las Positas Road 
Livermore, California 94551 
Tel:  925-449-2500  ♦  Fax:  925-449-2507 
Email:  sales@lstc.com 
Website:  www.lstc.com 
Disclaimer 
Technology 
Software 
Livermore 
Corporation 
1740 West Big Beaver Road 
Suite 100 
Troy, Michigan  48084 
Tel:  248-649-4728  ♦  Fax:  248-649-6328 
Copyright © 1992-2019 Livermore Software Technology Corporation.  All Rights Reserved. 
LS-DYNA®,  LS-OPT®  and  LS-PrePost®  are  registered  trademarks  of  Livermore  Software  Technology 
Corporation in the United States.  All other trademarks, product names and brand names belong to their 
respective owners. 
LSTC products are protected under  the following US patents:  7953578, 7945432, 7702494, 7702490, 7664623, 7660480, 
7657394, 7640146, 7613585, 7590514, 7533577, 7516053, 7499050, 7472602, 7428713, 7415400, 7395128, 7392163, 7386428, 
7386425, 7382367, 7308387, 7286972, 7167816, 8050897, 8069017, 7987143, 7996344, 8126684, 8150668, 8165856, 8180605, 
8190408,  8200464,  8296109,  8209157,  8271237,  8200458,  8306793,  Japan  patent  5090426  and  pending  patents 
applications. 
LSTC reserves the right to modify the material contained within this manual without prior notice. 
The information and examples included herein are for illustrative purposes only and are not intended to 
be exhaustive or all-inclusive.  LSTC assumes no liability  or responsibility  whatsoever for any direct  of 
indirect damages or inaccuracies of any type or nature that could be deemed to have resulted from the 
use of this manual. 
Any reproduction, in whole or in part, of this manual is prohibited without the prior written approval of 
LSTC.  All requests to reproduce the contents hereof should be sent to sales@lstc.com. 
AES.  Copyright © 2001, Dr Brian Gladman < brg@gladman.uk.net>, Worcester, UK.  All rights reserved. 
LICENSE TERMS 
The free distribution and use of this software in both source and binary form is allowed (with or without 
changes) provided that: 
1. 
2. 
3. 
distributions of this source code include the above copyright notice, this list of conditions and 
the following disclaimer; 
distributions in binary form include the above copyright notice, this list of conditions and the 
following disclaimer in the documentation and/or other associated materials; 
the copyright holder's name is not used to endorse products built using this software without 
specific written permission.  
DISCLAIMER 
This  software  is  provided  'as  is'  with  no  explicit  or  implied  warranties  in  respect  of  any  properties,
This file contains the code for implementing the key schedule for AES (Rijndael) for block and key sizes 
of 16, 24, and 32 bytes.
LS-DYNA Theory Manual 
Abstract 
1    
Abstract 
LS-DYNA  is  a  general  purpose  finite  element  code  for  analyzing  the  large 
deformation static and dynamic response of structures including structures coupled to 
fluids.    The  main  solution  methodology  is  based  on  explicit  time  integration.    An 
implicit  solver  is  currently  available  with  somewhat  limited  capabilities  including 
structural  analysis  and  heat  transfer.    A  contact-impact  algorithm  allows  difficult 
contact  problems  to  be  easily  treated  with  heat  transfer  included  across  the  contact 
interfaces.      By  a  specialization  of  this  algorithm,  such  interfaces  can  be  rigidly tied  to 
admit  variable  zoning  without  the  need  of  mesh  transition  regions.    Other  specializa-
tions, allow draw beads in metal stamping applications to be easily modeled simply by 
defining a line of nodes along the draw bead.  Spatial discretization is achieved by the 
use of four node tetrahedron and eight node solid elements, two node beam elements, 
three  and  four  node  shell  elements,  eight  node  solid  shell  elements,  truss  elements, 
membrane  elements,  discrete  elements,  and  rigid  bodies.    A  variety  of  element 
formulations  are  available  for  each  element  type.    Specialized  capabilities  for  airbags, 
sensors,  and  seatbelts  have  tailored  LS-DYNA  for  applications  in  the  automotive 
industry.    Adaptive  remeshing  is  available  for  shell  elements  and  is  widely  used  in 
sheet  metal  stamping  applications.    LS-DYNA  currently  contains  approximately  one-
hundred  constitutive  models  and  ten  equations-of-state  to  cover  a  wide  range  of 
material  behavior.    This  theoretical  manual  has  been  written  to  provide  users  and 
potential users with insight into the mathematical and physical basis of the code.
LS-DYNA Theory Manual 
History of LS-DYNA 
2    
History of LS-DYNA 
The  origin  of  LS-DYNA  dates  back  to  the  public  domain  software,  DYNA3D, 
which  was  developed  in  the  mid-seventies  at  the  Lawrence  Livermore  National 
Laboratory.  The first version of DYNA3D [Hallquist 1976a] was released in 1976 with 
constant stress 4- or 8-node solid elements, 16- and 20-node solid elements with 2 × 2 × 
2  Gaussian  quadrature,  3,  4,  and  8-node  membrane  elements,  and  a  2-node  cable 
element.    A  nodal  constraint  contact-impact  interface  algorithm  [Hallquist  1977]  was 
available.    On  the  Control  Data  CDC-7600,  a  supercomputer  in  1976,  the  speed  of  the 
code  varied  from  36 minutes  per  106  mesh  cycles  with  4-8  node  solids  to  180  minutes 
per 106 mesh cycles with 16 and 20 node solids.  Without hourglass control to prevent 
formation of non-physical zero energy deformation modes, constant stress solids were 
processed  at  12  minutes  per  106  mesh  cycles.    A  moderate  number  of  very  costly 
solutions  were  obtained  with  this  version  of  DYNA3D  using  16-  and  20-node  solids.  
Hourglass  modes  combined  with  the  procedure  for  computing  the  time  step  size 
prevented us from obtaining solutions with constant stress elements. 
In  this  early  development,  several  things  became  apparent. 
  Hourglass 
deformation  modes  of  the  constant  stress  elements  were  invariably  excited  by  the 
contact-impact algorithm, showing that a new sliding interface algorithm was needed.  
Higher order elements seemed to be impractical for shock wave propagation because of 
numerical  noise  resulting  from  the  ad  hoc  mass  lumping  necessary  to  generate  a 
diagonal  mass  matrix.    Although  the  lower  frequency  structural  response  was 
accurately  computed  with  these  elements,  their  high  computer  cost  made  analysis  so 
expensive as to be impractical.  It was obvious that realistic three-dimensional structural 
calculations were possible, if and only if the under-integrated eight node constant stress 
solid element could be made to function.  This implied a need for a much better sliding 
interface  algorithm,  a  more  cost-effective  hourglass  control,  more  optimal  program-
ming,  and  a  machine  much  faster  than  the  CDC-7600.    This  latter  need  was  fulfilled 
several years later when LLNL took deliver of its first CRAY-1.  At this time, DYNA3D 
was completely rewritten.
History of LS-DYNA 
LS-DYNA Theory Manual 
The  next  version,  released  in  1979,  achieved  the  aforementioned  goals.    On  the 
CRAY the vectorized speed was 50 times  faster, 0.67 minutes per  million mesh cycles.  
A  symmetric,  penalty-based,  contact-impact  algorithm  was  considerably  faster  in 
execution speed and exceedingly reliable.  Due to lack of use, the membrane and cable 
elements were stripped and all higher order elements were eliminated as well.  Wilkins’ 
finite difference equations [Wilkins et al.  1974] were implemented in unvectorized form 
in an overlay to compare their performance with the finite element method.  The finite 
difference  algorithm  proved  to  be  nearly  two  times  more  expensive  than  the  finite 
element  approach  (apart  from  vectorization)  with  no  compensating  increase  in 
accuracy, and was removed in the next code update. 
The  1981  version  [Hallquist  1981a]  evolved  from  the  1979  version.    Nine 
additional material models were added to allow a much broader range of problems to 
be  modeled  including  explosive-structure  and  soil-structure  interactions.    Body  force 
loads were implemented for angular velocities and base accelerations.  A link was also 
established  from  the  3D  Eulerian  code  JOY  [Couch,  et.    al.,  1983]  for  studying  the 
structural response to impacts by penetrating projectiles.  An option was provided for 
storing element data on disk thereby doubling the capacity of DYNA3D. 
The  1982  version  of  DYNA3D  [Hallquist  1982]  accepted  DYNA2D  [Hallquist 
1980]  material  input  directly.    The  new  organization  was  such  that  equations  of  state 
and  constitutive  models  of  any  complexity  could  be  easily  added.    Complete 
vectorization of the material models had been nearly achieved with about a 10 percent 
increase in execution speed over the 1981 version. 
In the 1986 version of DYNA3D [Hallquist and Benson 1986], many new features 
were  added,  including  beams,  shells,  rigid  bodies,  single  surface  contact,  interface 
friction,  discrete  springs  and  dampers,  optional  hourglass  treatments,  optional  exact 
volume integration, and VAX/VMS, IBM, UNIX, COS operating systems compatibility, 
that greatly expanded its range of applications.  DYNA3D thus became the first code to 
have a general single surface contact algorithm. 
In  the  1987  version  of  DYNA3D  [Hallquist  and  Benson  1987]  metal  forming 
simulations  and  composite  analysis  became  a  reality.    This  version  included  shell 
thickness changes, the Belytschko-Tsay shell element [Belytschko and Tsay, 1981], and 
dynamic  relaxation.    Also  included  were  non-reflecting  boundaries,  user  specified 
integration rules for shell and beam elements, a layered composite damage model, and 
single point constraints. 
New capabilities added in the 1988 DYNA3D [Hallquist 1988] version included a 
cost  effective  resultant  beam  element,  a  truss  element,  a  C0  triangular  shell,  the  BCIZ 
triangular  shell  [Bazeley  et  al.,  1965],  mixing  of  element  formulations  in  calculations, 
composite  failure  modeling  for  solids,  noniterative  plane  stress  plasticity,  contact 
surfaces  with  spot  welds,  tiebreak  sliding  surfaces,  beam  surface  contact,  finite
LS-DYNA Theory Manual 
History of LS-DYNA 
stonewalls,  stonewall  reaction  forces,  energy  calculations  for  all  elements,  a  crushable 
foam constitutive model, comment cards in the input, and one-dimensional slidelines. 
In  1988  the  Hallquist  began  working  half-time  at  LLNL  to  devote  more  time  to 
the development and support of LS-DYNA for automotive applications.  By the end of 
1988  it  was  obvious  that  a  much  more  concentrated  effort  would  be  required  in  the 
development of LS-DYNA if problems in crashworthiness were to be properly solved; 
therefore,  at  the  start  of  1989  the  Hallquist  resigned  from  LLNL  to  continue  code 
development  full  time  at  Livermore  Software  Technology  Corporation.    The  1989 
version introduced many enhanced capabilities including a one-way treatment of slide 
surfaces  with  voids  and  friction;  cross-sectional  forces  for  structural  elements;  an 
optional  user  specified  minimum  time  step  size  for  shell  elements  using  elastic  and 
elastoplastic  material  models;  nodal  accelerations  in  the  time  history  database;  a 
compressible  Mooney-Rivlin  material  model;  a  closed-form  update  shell  plasticity 
model;  a  general  rubber  material  model;  unique  penalty  specifications  for  each  slide 
surface;  external  work  tracking;  optional  time  step  criterion  for  4-node  shell  elements; 
and  internal  element  sorting  to  allow  full  vectorization  of  right-hand-side  force 
assembly. 
2.1  Features add in 1989-1990 
Throughout  the  past  decade,  considerable  progress  has  been  made  as  may  be 
seen  in  the  chronology  of  the  developments  which  follows.    During  1989  many 
extensions  and  developments  were  completed,  and  in  1990  the  following  capabilities 
were delivered to users: 
•  arbitrary node and element numbers, 
•  fabric model for seat belts and airbags, 
•  composite glass model, 
•  vectorized type 3 contact and single surface contact, 
•  many more I/O options, 
•  all shell materials available for 8 node brick shell, 
•  strain rate dependent plasticity for beams, 
•  fully vectorized iterative plasticity, 
• 
interactive graphics on some computers, 
•  nodal damping, 
•  shell thickness taken into account in shell type 3 contact, 
•  shell thinning accounted for in type 3 and type 4 contact, 
•  soft stonewalls,
History of LS-DYNA 
LS-DYNA Theory Manual 
•  print suppression option for node and element data, 
•  massless truss elements, rivets – based on equations of rigid body dynamics, 
•  massless  beam  elements,  spot  welds  –  based  on  equations  of  rigid  body 
dynamics, 
•  expanded databases with more history variables and integration points, 
•  force limited resultant beam, 
•  rotational spring and dampers, local coordinate systems for discrete elements, 
•  resultant plasticity for C0 triangular element, 
•  energy dissipation calculations for stonewalls, 
•  hourglass energy calculations for solid and shell elements, 
•  viscous and Coulomb friction with arbitrary variation over surface, 
•  distributed loads on beam elements, 
•  Cowper and Symonds strain rate model, 
•  segmented stonewalls, 
•  stonewall Coulomb friction, 
•  stonewall energy dissipation, 
•  airbags (1990), 
•  nodal rigid bodies, 
•  automatic sorting of triangular shells into C0 groups, 
•  mass scaling for quasi static analyses, 
•  user defined subroutines, 
•  warpage checks on shell elements, 
•  thickness consideration in all contact types, 
•  automatic orientation of contact segments, 
•  sliding interface energy dissipation calculations, 
•  nodal force and energy database for applied boundary conditions, 
•  defined stonewall velocity with input energy calculations, 
2.2  Options added in 1991-1992 
•  rigid/deformable material switching, 
•  rigid bodies impacting rigid walls,
LS-DYNA Theory Manual 
History of LS-DYNA 
•  strain-rate effects in metallic honeycomb model 26, 
•  shells and beams interfaces included for subsequent component analyses, 
•  external work computed for prescribed displacement/velocity/accelerations, 
• 
linear constraint equations, 
•  MPGS database, 
•  MOVIE database, 
•  Slideline interface file, 
•  automated contact input for all input types, 
•  automatic single surface contact without element orientation, 
•  constraint technique for contact, 
•  cut planes for resultant forces, 
•  crushable cellular foams, 
•  urethane foam model with hysteresis, 
•  subcycling, 
•  friction in the contact entities, 
•  strains computed and written for the 8 node thick shells, 
•  “good” 4 node tetrahedron solid element with nodal rotations, 
•  8 node solid element with nodal rotations, 
•  2 × 2 integration for the membrane element, 
•  Belytschko-Schwer integrated beam, 
•  thin-walled Belytschko-Schwer integrated beam, 
• 
improved LS-DYNA database control, 
•  null material for beams to display springs and seatbelts in TAURUS, 
•  parallel implementation on Cray and SGI computers, 
•  coupling to rigid body codes, 
•  seat belt capability. 
2.3  Options added in 1993-1994 
•  Arbitrary Lagrangian Eulerian brick elements, 
•  Belytschko-Wong-Chiang quadrilateral shell element, 
•  Warping stiffness in the Belytschko-Tsay shell element,
History of LS-DYNA 
LS-DYNA Theory Manual 
•  Fast Hughes-Liu shell element, 
•  Fully integrated brick shell element, 
•  Discrete 3D beam element, 
•  Generalized dampers, 
•  Cable modeling, 
•  Airbag reference geometry, 
•  Multiple jet model, 
•  Generalized joint stiffnesses, 
•  Enhanced rigid body to rigid body contact, 
•  Orthotropic rigid walls, 
•  Time zero mass scaling, 
•  Coupling with USA (Underwater Shock Analysis), 
•  Layered spot welds with failure based on resultants or plastic strain, 
•  Fillet welds with failure, 
•  Butt welds with failure, 
•  Automatic eroding contact, 
•  Edge-to-edge contact, 
•  Automatic mesh generation with contact entities, 
•  Drawbead modeling, 
•  Shells constrained inside brick elements, 
•  NIKE3D coupling for springback, 
•  Barlat’s anisotropic plasticity, 
•  Superplastic forming option, 
•  Rigid body stoppers, 
•  Keyword input, 
•  Adaptivity, 
•  First MPP (Massively Parallel) version with limited capabilities. 
•  Built in least squares fit for rubber model constitutive constants, 
•  Large hystersis in hyperelastic foam, 
•  Bilhku/Dubois foam model, 
•  Generalized rubber model,
LS-DYNA Theory Manual 
History of LS-DYNA 
2.4  Version 936 
New options added to version 936 in 1995 include: 
•  Belytschko - Leviathan Shell 
•  Automatic switching between rigid and deformable bodies. 
•  Accuracy  on  SMP  machines  to  give  identical  answers  on  one,  two  or  more 
processors.  
•  Local coordinate systems for cross-section output can now be specified. 
•  Null material for shell elements. 
•  Global body force loads now may be applied to a subset of materials. 
•  User defined loading subroutine. 
•  Improved interactive graphics. 
•  New initial velocity options for specifying rotational velocities.  
•  Geometry  changes  after  dynamic  relaxation  can  be  considered  for  initial 
velocities.   
•  Velocities may also be specified by using material or part ID’s. 
•  Improved speed of brick element hourglass force and energy calculations. 
•  Pressure outflow boundary conditions have been added for the ALE options. 
•  More user control for hourglass control constants for shell elements. 
•  Full vectorization in constitutive models for foam, models 57 and 63. 
•  Damage mechanics plasticity model, material 81, 
•  General linear viscoelasticity with 6 term prony series. 
•  Least squares fit for viscoelastic material constants. 
•  Table definitions for strain rate effects in material type 24. 
•  Improved treatment of free flying nodes after element failure. 
•  Automatic  projection  of  nodes  in  CONTACT_TIED  to  eliminate  gaps  in  the 
surface.   
•  More user control over contact defaults. 
•  Improved interpenetration warnings printed in automatic contact. 
•  Flag for using actual shell thickness in single surface contact logic rather than the 
default.  
•  Definition by exempted part ID’s. 
•  Airbag to Airbag venting/segmented airbags are now supported.
History of LS-DYNA 
LS-DYNA Theory Manual 
•  Airbag reference geometry speed improvements by using the reference geometry 
for the time step size calculation.  
•  Isotropic airbag material may now be directly for cost efficiency. 
•  Airbag fabric material damping is now specified as the ratio of critical damping.   
•  Ability  to  attach  jets  to  the  structure  so  the  airbag,  jets,  and  structure  to  move 
together. 
•  PVM 5.1 Madymo coupling is available. 
•  Meshes are generated within LS-DYNA3D for all standard contact entities. 
•  Joint damping for translational motion.     
•  Angular  displacements,  rates  of  displacements,  damping  forces,  etc. 
  in 
JNTFORC file. 
•  Link between LS-NIKE3D to LS-DYNA3D via *INITIAL_STRESS keywords.  
•  Trim curves for metal forming springback. 
•  Sparse equation solver for springback. 
•  Improved mesh generation for IGES and VDA provides a mesh that can directly 
be used to model tooling in metal stamping analyses. 
2.5  Version 940 
New options added to Version 940 in 1996 and 1997: 
•  Part/Material ID’s may be specified with 8 digits. 
•  Rigid body motion can be prescribed in a local system fixed to the rigid body. 
•  Nonlinear least squares fit available for the Ogden rubber model. 
•  Lease squares fit to the relaxation curves for the viscoelasticity in rubber. 
•  Fu-Chang rate sensitive foam. 
•  6 term Prony series expansion for rate effects in model 57-now 73 
•  Viscoelastic material model 76 implemented for shell elements. 
•  Mechanical threshold stress (MTS) plasticity model for rate effects. 
•  Thermoelastic-plastic material model for Hughes-Liu beam element. 
•  Ramberg-Osgood soil model 
•  Invariant local coordinate systems for shell elements are optional. 
•  Second order accurate stress updates. 
•  Four-noded, linear, tetrahedron element.
LS-DYNA Theory Manual 
History of LS-DYNA 
•  Co-rotational solid element for foam that can invert without stability problems. 
•  Improved speed in rigid body to rigid body contacts.   
•  Improved searching for the a_3, a_5 and a10 contact types.   
•  Invariant results on shared memory parallel machines with the a_n contact types. 
•  Thickness offsets in type 8 and 9 tie break contact algorithms.  
•  Bucket sort frequency can be controlled by a load curve for airbag applications. 
•  In automatic contact each part ID in the definition may have unique: 
◦  Static coefficient of friction 
◦  Dynamic coefficient of friction 
◦  Exponential decay coefficient 
◦  Viscous friction coefficient 
◦  Optional contact thickness 
◦  Optional thickness scale factor 
◦  Local penalty scale factor 
•  Automatic beam-to-beam, shell edge-to-beam, shell edge-to-shell edge and single 
surface contact algorithm. 
•  Release criteria may be a multiple of the shell thickness in types a_3, a_5, a10, 13, 
and 26 contact. 
•  Force  transducers  to  obtain  reaction  forces  in  automatic  contact  definitions.  
Defined manually via segments, or automatically via part ID’s. 
•  Searching depth can be defined as a function of time. 
•  Bucket sort frequency can be defined as a function of time. 
•  Interior contact for solid (foam) elements to prevent "negative volumes." 
•  Locking joint 
•  Temperature dependent heat capacity added to Wang-Nefske inflator models. 
•  Wang  Hybrid  inflator  model  [Wang,  1996]  with  jetting  options  and  bag-to-bag 
venting. 
•  Aspiration included in Wang’s hybrid model [Nucholtz, Wang, Wylie, 1996]. 
•  Extended Wang’s hybrid inflator with a quadratic temperature variation for heat 
capacities [Nusholtz, 1996].  
•  Fabric porosity added as part of the airbag constitutive model. 
•  Blockage of vent holes and fabric in contact with structure or itself considered in 
venting with leakage of gas.
History of LS-DYNA 
LS-DYNA Theory Manual 
•  Option to delay airbag liner with using the reference geometry until the reference 
area is reached. 
•  Birth time for the reference geometry. 
•  Multi-material Euler/ALE fluids,  
◦  2nd order accurate formulations.  
◦  Automatic coupling to shell, brick, or beam elements 
◦  Coupling using LS-DYNA contact options. 
◦  Element with fluid + void and void material 
◦  Element with multi-materials and pressure equilibrium 
•  Nodal inertia tensors. 
•  2D plane stress, plane strain, rigid, and axisymmetric elements 
•  2D plane strain shell element 
•  2D axisymmetric shell element. 
•  Full contact support in 2D, tied, sliding only, penalty and constraint techniques. 
•  Most material types supported for 2D elements. 
•  Interactive remeshing and graphics options available for 2D. 
•  Subsystem definitions for energy and momentum output.  and many more 
enhancements not mentioned above. 
2.6  Version 950 
Capabilities added during 1997-1998 in Version 950 include: 
•  Adaptive refinement can be based on tooling curvature with FORMING contact. 
•  The  display  of  draw  beads  is  now  possible  since  the  draw  bead  data  is  output 
into the d3plot database. 
•  An  adaptive  box  option,  *DEFINE_BOX_ADAPTIVE,  allows  control  over  the 
refinement level and location of elements to be adapted. 
•  A  root  identification  file,  adapt.rid,  gives  the  parent  element  ID  for  adapted 
elements. 
•  Draw  bead  box  option,  *DEFINE_BOX_DRAWBEAD,  simplifies  draw  bead 
input. 
•  The  new  control  option,  CONTROL_IMPLICIT,  activates  an  implicit  solution 
scheme. 
•  2D Arbitrary-Lagrangian-Eulerian elements.
LS-DYNA Theory Manual 
History of LS-DYNA 
•  2D automatic contact is defined by listing part ID's. 
•  2D  r-adaptivity  for  plane  strain  and  axisymmetric  forging  simulations  is 
available. 
•  2D automatic non-interactive rezoning as in LS-DYNA2D. 
•  2D  plane  strain  and  axisymmetric  element  with  2 ×  2  selective-reduced 
integration are implemented. 
•  Implicit 2D solid and plane strain elements are available. 
•  Implicit 2D contact is available. 
•  The  new  keyword,  *DELETE_CONTACT_2DAUTO,  allows  the  deletion  of  2D 
automatic contact definitions. 
•  The keyword, *LOAD_BEAM is added for pressure boundary conditions on 2D 
elements. 
•  A viscoplastic strain rate option is available for materials: 
◦  *MAT_PLASTIC_KINEMATIC 
◦  *MAT_JOHNSON_COOK 
◦  *MAT_POWER_LAW_PLASTICITY 
◦  *MAT_STRAIN_RATE_DEPENDENT_PLASTICITY 
◦  *MAT_PIECEWISE_LINEAR_PLASTICITY  
◦  *MAT_RATE_SENSITIVE_POWERLAW_PLASTICITY 
◦  *MAT_ZERILLI-ARMSTRONG 
◦  *MAT_PLASTICITY_WITH_DAMAGE 
◦  *MAT_PLASTICITY_COMPRESSION_TENSION  
•  Material  model,  *MAT_PLASTICITY_WITH_DAMAGE,  has  a  piecewise  linear 
damage curve given by a load curve ID. 
•  The  Arruda-Boyce  hyper-viscoelastic  rubber  model  is  available,  see  *MAT_AR-
RUDA_BOYCE. 
•  Transverse-anisotropic-viscoelastic material for heart tissue, see *MAT_HEART_-
TISSUE. 
•  Lung hyper-viscoelastic material, see *MAT_LUNG_TISSUE. 
•  Compression/tension  plasticity  model,  see  *MAT_PLASTICITY_COMPRES-
SION_TENSION.  
•  The  Lund  strain  rate  model,  *MAT_STEINBERG_LUND,  is  added  to  Steinberg-
Guinan plasticity model. 
•  Rate  sensitive  foam  model,  *MAT_FU_CHANG_FOAM,  has  been  extended  to 
include engineering strain rates, etc.
History of LS-DYNA 
LS-DYNA Theory Manual 
•  Model,  *MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY,  is  added  for 
modeling the failure of aluminum. 
•  Material model, *MAT_SPECIAL_ORTHOTROPIC, added for television shadow 
mask problems. 
•  Erosion strain is implemented for material type, *MAT_BAMMAN_DAMAGE. 
•  The  equation  of  state,  *EOS_JWLB,  is  available  for  modeling  the  expansion  of 
explosive gases. 
•  The  reference  geometry  option  is  extended  for  foam  and  rubber  materials  and 
can be used for stress initialization, see *INITIAL_FOAM_REFERENCE_GEOM-
ETRY. 
•  A  vehicle  positioning  option  is  available  for  setting  the  initial  orientation  and 
velocities, see *INITIAL_VEHICLE_KINEMATICS. 
•  A  boundary  element  method  is  available  for  incompressible  fluid  dynamics 
problems. 
•  The  thermal  materials  work  with  instantaneous  coefficients  of  thermal  expan-
sion: 
◦  *MAT_ELASTIC_PLASTIC_THERMAL 
◦  *MAT_ORTHOTROPIC_THERMAL 
◦  *MAT_TEMPERATURE_DEPENDENT_ORTHOTROPIC  
◦  *MAT_ELASTIC_WITH_VISCOSITY. 
•  Airbag interaction flow rate versus pressure differences. 
•  Contact segment search option, [bricks first optional] 
•  A through thickness Gauss integration rule with 1-10 points is available for shell 
elements.  Previously, 5 were available. 
•  Shell element formulations can be changed in a full deck restart. 
•  The tied interface which is based on constraint equations, TIED_SURFACE_TO_-
SURFACE, can now fail with FAILURE option. 
•  A general failure criteria for solid elements is independent of the material type, 
see *MAT_ADD_EROSION 
•  Load curve control can be based on thinning and a flow limit diagram, see *DE-
FINE_CURVE_FEEDBACK. 
•  An option to filter the spotweld resultant forces prior to checking for failure has 
been  added  the  option,  *CONSTRAINED_SPOTWELD,  by  appending,_FIL-
TERED_FORCE, to the keyword. 
•  Bulk viscosity is available for shell types 1, 2, 10, and 16.
LS-DYNA Theory Manual 
History of LS-DYNA 
•  When  defining  the  local  coordinate  system  for  the  rigid  body  inertia  tensor  a 
local coordinate system ID can be used.  This simplifies dummy positioning. 
•  Prescribing displacements, velocities, and accelerations is now possible for rigid 
body nodes. 
•  One-way flow is optional for segmented airbag interactions. 
•  Pressure time history input for airbag type, LINEAR_FLUID, can be used. 
•  An option is available to independently scale system damping by part ID in each 
of the global directions. 
•  An option is available to independently scale global system damping in each of 
the global directions. 
•  Added option to constrain global DOF along lines parallel with the global axes.  
The  keyword  is  *CONSTRAINED_GLOBAL.  This  option  is  useful  for  adaptive 
remeshing. 
•  Beam end code releases are available, see *ELEMENT_BEAM. 
•  An  initial  force  can  be  directly  defined  for  the  cable  material,  *MAT_CABLE_-
DISCRETE_BEAM.    The  specification  of  slack  is  not  required  if  this  option  is 
used. 
•  Airbag pop pressure can be activated by accelerometers. 
•  Termination  may  now  be  controlled  by  contact,  via  *TERMINATION_CON-
TACT. 
•  Modified  shell  elements  types  8,  10  and  the  warping  stiffness  option  in  the 
Belytschko-Tsay  shell  to  ensure  orthogonality  with  rigid  body  motions  in  the 
event that the shell is badly warped.  This is optional in the Belytschko-Tsay shell 
and the type 10 shell. 
•  A  one  point  quadrature  brick  element  with  an  exact  hourglass  stiffness  matrix 
has been implemented for implicit and explicit calculations. 
•  Automatic  file  length  determination  for  d3plot  binary  database  is  now  imple-
mented.    This  insures  that  at  least  a  single  state  is  contained  in  each  d3plot  file 
and eliminates the problem with the states being split between files. 
•  The  dump  files,  which  can  be  very  large,  can  be  placed  in  another  directory  by 
specifying d=/home/user /test/d3dump on the execution line. 
•  A print flag controls the output of data into the MATSUM and RBDOUT files by 
part  ID's.    The  option,  PRINT,  has  been  added  as  an  option  to  the  *PART  key-
word. 
•  Flag  has  been  added  to  delete  material  data  from  the  d3thdt  file.    See  *DATA-
BASE_EXTENT_BINARY  and  column  25  of  the  19th  control  card  in  the  struc-
tured input.
History of LS-DYNA 
LS-DYNA Theory Manual 
•  After  dynamic  relaxation  completes,  a  file  is  written  giving  the  displaced  state 
which can be used for stress initialization in later runs. 
2.7  Version 960 
Capabilities  added  during  1998-2000  in  Version  960.    Most  new  capabilities  work  on 
both the MPP and SMP versions; however, the capabilities that are implemented for the 
SMP version only, which were not considered critical for this release, are flagged below.  
These  SMP  unique  capabilities  are  being  extended  for  MPP  calculations  and  will  be 
available in the near future.  The implicit capabilities for MPP require the development 
of  a  scalable  eigenvalue  solver,  which  is  under  development  for  a  later  release  of  LS-
DYNA.   
•  Incompressible  flow  solver  is  available.    Structural  coupling  is  not  yet  imple-
mented. 
•  Adaptive  mesh  coarsening  can  be  done  before  the  implicit  spring  back  calcula-
tion in metal forming applications. 
•  Two-dimensional  adaptivity  can  be  activated  in  both  implicit  and  explicit 
calculations.  (SMP version only) 
•  An internally generated smooth load curve for metal forming tool motion can be 
activated with the keyword: *DEFINE_CURVE_SMOOTH. 
•  Torsional forces can be carried through the deformable spot welds by using the 
contact  type:  *CONTACT_SPOTWELD_WITH_TORSION  (SMP  version  only 
with a high priority for the MPP version if this option proves to be stable.) 
•  Tie  break  automatic  contact  is  now  available  via  the  *CONTACT_AUTOMAT-
IC_..._TIEBREAK options.  This option can be used for glued panels.  (SMP only) 
•  *CONTACT_RIGID_SURFACE  option  is  now  available  for  modeling  road 
surfaces (SMP version only). 
•  Fixed rigid walls PLANAR and PLANAR_FINITE are represented in the binary 
output file by a single shell element. 
•  Interference fits can be modeled with the INTERFERENCE option in contact. 
•  A layered shell theory is implemented for several constitutive models including 
the composite models to more accurately represent the shear stiffness of laminat-
ed shells. 
•  Damage  mechanics  is  available  to  smooth  the  post-failure  reduction  of  the 
resultant forces in the constitutive model *MAT_SPOTWELD_DAMAGE. 
•  Finite  elastic  strain  isotropic  plasticity  model  is  available  for  solid  elements.  
*MAT_FINITE_ELASTIC_STRAIN_PLASTICITY. 
•  A shape memory alloy material is available: *MAT_SHAPE_MEMORY.
LS-DYNA Theory Manual 
History of LS-DYNA 
•  Reference  geometry  for  material,  *MAT_MODIFIED_HONEYCOMB,  can  be  set 
at arbitrary relative volumes or when the time step size reaches a limiting value.  
This option is now available for all element types including the fully integrated 
solid element. 
•  Non  orthogonal  material  axes  are  available  in  the  airbag  fabric  model.    See 
*MAT_FABRIC. 
•  Other new constitutive models include for the beam elements: 
◦  *MAT_MODIFIED_FORCE_LIMITED 
◦  *MAT_SEISMIC_BEAM 
◦  *MAT_CONCRETE_BEAM 
•  for shell and solid elements: 
◦  *MAT_ELASTIC_VISCOPLASTIC_THERMAL 
•  for the shell elements: 
◦  *MAT_GURSON 
◦  *MAT_GEPLASTIC_SRATE2000 
◦  *MAT_ELASTIC_VISCOPLASTIC_THERMAL 
◦  *MAT_COMPOSITE_LAYUP 
◦  *MAT_COMPOSITE_LAYUP 
◦  *MAT_COMPOSITE_direct  
•  for the solid elements: 
◦  *MAT_JOHNSON_HOLMQUIST_CERAMICS 
◦  *MAT_JOHNSON_HOLMQUIST_CONCRETE 
◦  *MAT_INV_HYPERBOLIC_SIN 
◦  *MAT_UNIFIED_CREEP 
◦  *MAT_SOIL_BRICK 
◦  *MAT_DRUCKER_PRAGER 
◦  *MAT_RC_SHEAR_WALL 
•  and for all element options a very fast and efficient version of the Johnson-Cook 
plasticity model is available: 
◦  *MAT_SIMPLIFIED_JOHNSON_COOK 
•  A  fully  integrated  version  of  the  type  16  shell  element  is  available  for  the 
resultant constitutive models.
History of LS-DYNA 
LS-DYNA Theory Manual 
•  A  nonlocal  failure  theory  is  implemented  for  predicting  failure  in  metallic 
materials.  The keyword *MAT_NONLOCAL activates this option for a subset of 
elastoplastic constitutive models. 
•  A  discrete  Kirchhoff  triangular  shell  element  (DKT)  for  explicit  analysis  with 
three  in  plane  integration  points  is  flagged  as  a  type  17  shell  element.    This 
element has much better bending behavior than the C0 triangular element. 
•  A discrete Kirchhoff linear triangular and quadrilaterial shell element is available 
as a type 18 shell.  This shell is for extracting normal modes and static analysis. 
•  A C0 linear 4-node quadrilaterial shell element is implemented as element type 
20 with drilling stiffness for normal modes and static analysis. 
•  An assumed strain linear brick element is available for normal modes and statics. 
•  The  fully  integrated  thick  shell  element  has  been  extended  for  use  in  implicit 
calculations. 
•  A fully integrated thick shell element based on an assumed strain formulation is 
now available.  This element uses a full 3D constitutive model which includes the 
normal  stress  component  and,  therefore,  does  not  use  the  plane  stress  assump-
tion. 
•  The  4-node  constant  strain  tetrahedron  element  has  been  extended  for  use  in 
implicit calculations. 
•  Relative  damping  between  parts  is  available,  see  *DAMPING_RELATIVE  (SMP 
only).   
•  Preload forces are can be input for the discrete beam elements. 
•  Objective  stress  updates  are  implemented  for  the  fully  integrated  brick  shell 
element. 
•  Acceleration time histories can be prescribed for rigid bodies. 
•  Prescribed motion for nodal rigid bodies is now possible. 
•  Generalized  set  definitions,  i.e.,  SET_SHELL_GENERAL  etc.    provide  much 
flexibility in the set definitions. 
•  The command "sw4." will write a state into the dynamic relaxation file, D3DRLF, 
during the dynamic relaxation phase if the d3drlf file is requested in the input. 
•  Added  mass  by  PART  ID  is  written  into  the  matsum  file  when  mass  scaling  is 
used to maintain the time step size, (SMP version only). 
•  Upon termination due to a large mass increase during a mass scaled calculation a 
print summary of 20 nodes with the maximum added mass is printed. 
•  Eigenvalue  analysis  of  models  containing  rigid  bodies  is  now  available  using 
BCSLIB-EXT solvers from Boeing.  (SMP version only).
LS-DYNA Theory Manual 
History of LS-DYNA 
•  Second order stress updates can be activated by part ID instead of globally on the 
*CONTROL_ACCURACY input. 
•  Interface  frictional  energy  is  optionally  computed  for  heat  generation  and  is 
output into the interface force file (SMP version only). 
•  The  interface  force  binary  database  now  includes  the  distance  from  the  contact 
surface for the FORMING contact options.  This distance is given after the nodes 
are detected as possible contact candidates.  (SMP version only). 
•  Type 14 acoustic brick element is implemented.  This element is a fully integrated 
version of type 8, the acoustic element (SMP version only). 
•  A  flooded  surface  option  for  acoustic  applications  is  available  (SMP  version 
only). 
•  Attachment nodes can be defined for rigid bodies.  This option is useful for NVH 
applications. 
•  CONSTRAINED_POINTS tie any two points together.  These points must lie on 
a shell element. 
•  Soft constraint is available for edge-to-edge contact in type 26 contact. 
•  CONSTAINED_INTERPOLATION  option  for  beam  to  solid  interfaces  and  for 
spreading the mass and loads.  (SMP version only). 
•  A database option has been added that allows the output of added mass for shell 
elements instead of the time step size. 
•  A  new  contact  option  allows  the  inclusion  of  all  internal  shell  edges  in  contact 
type *CONTACT_GENERAL, type 26.  This option is activated by adding INTE-
RIOR option. 
•  A  new  option  allows  the  use  deviatoric  strain  rates  rather  than  total  rates  in 
material model 24 for the Cowper-Symonds rate model. 
•  The  CADFEM  option  for  ASCII  databases  is  now  the  default.    Their  option 
includes more significant figures in the output files. 
•  When  using  deformable  spot  welds,  the  added  mass  for  spot  welds  is  now 
printed for the case where global mass scaling is activated.  This output is in the 
log file, d3hsp file, and the messag file. 
•  Initial  penetration  warnings  for  edge-to-edge  contact  are  now  written  into  the 
MESSAG file and the D3HSP file. 
•  Each compilation of LS-DYNA is given a unique version number. 
•  Finite length discrete beams with various local axes options are now available for 
material types 66, 67, 68, 93, and 95.  In this implementation the absolute value of 
SCOOR must be set to 2 or 3 in the *SECTION_BEAM input. 
•  New discrete element constitutive models are available:
History of LS-DYNA 
LS-DYNA Theory Manual 
◦  *MAT_ELASTIC_SPRING_DISCRETE_BEAM 
◦  *MAT_INELASTIC_SPRING_DISCRETE_BEAM 
◦  *MAT_ELASTIC_6DOF_SPRING_DISCRETE_BEAM 
◦  *MAT_INELASTIC_6DOF_SPRING_DISCRETE_BEAM 
The latter two can be used as finite length beams with local coordinate systems. 
•  Moving  SPC's  are  optional  in  that  the  constraints  are  applied  in  a  local  system 
that rotates with the 3 defining nodes. 
•  A moving local coordinate system, CID, can be used to determine orientation of 
discrete beam elements.  
•  Modal  superposition  analysis  can  be  performed  after  an  eigenvalue  analysis.  
Stress recovery is based on type 18 shell and brick (SMP only). 
•  Rayleigh damping input factor is now input as a fraction of critical damping, i.e. 
0.10.  The  old  method  required  the  frequency  of  interest  and  could  be  highly 
unstable for large input values. 
•  Airbag option "SIMPLE_PRESSURE_VOLUME" allows for the constant CN to be 
replaced  by  a  load  curve  for  initialization.    Also,  another  load  curve  can  be 
defined  which  allows  CN  to  vary  as  a  function  of  time  during  dynamic  relaxa-
tion.  After dynamic relaxation CN can be used as a fixed constant or load curve. 
•  Hybrid inflator model utilizing CHEMKIN and NIST databases is now available.  
Up to ten gases can be mixed. 
•  Option to track initial penetrations has been added in the automatic SMP contact 
types  rather  than  moving  the  nodes  back  to  the  surface.    This  option  has  been 
available  in  the  MPP  contact  for  some  time.    This  input  can  be  defined  on  the 
fourth card of the *CONTROL_CONTACT input and on each contact definition 
on the third optional card in the *CONTACT definitions. 
•  If the average acceleration flag is active, the  average acceleration for rigid body 
nodes  is  now  written  into  the  d3thdt  and  nodout  files.    In  previous  versions  of 
LS-DYNA, the accelerations on rigid nodes were not averaged. 
•  A  capability  to  initialize  the  thickness  and  plastic  strain  in  the  crash  model  is 
available  through  the  option  *INCLUDE_STAMPED_PART,  which  takes  the 
results  from  the  LS-DYNA  stamping  simulation  and  maps  the  thickness  and 
strain distribution onto the same part with a different mesh pattern. 
•  A  capability  to  include  finite  element  data  from  other  models  is  available 
through the option, *INCLUDE_TRANSFORM.  This option will take the model 
defined in an INCLUDE file: offset all ID's; translate, rotate, and scale the coordi-
nates; and transform the constitutive constants to another set of units.
LS-DYNA Theory Manual 
History of LS-DYNA 
2.8  Version 970 
Many new capabilities were added during 2001-2002 to create version 970 of LS-DYNA.  
Some of the new features, which are also listed below, were also added to later releases 
of version 960.  Most new explicit capabilities work for both the MPP and SMP versions; 
however,  the  implicit  capabilities  for  MPP  require  the  development  of  a  scalable 
eigenvalue  solver  and  a  parallel  implementation  of  the  constraint  equations  into  the 
global matrices.   This work is underway.  A later release of version 970 is planned that 
will be scalable for implicit solutions. 
•  MPP  decomposition  can  be  controlled  using  *CONTROL_MPP_DECOMPOSI-
TION commands in the input deck. 
•  The  MPP  arbitrary  Lagrangian-Eulerian  fluid  capability  now  works  for  airbag 
deployment in both SMP and MPP calculations. 
•  Euler-to-Euler  coupling 
is  now  available  through  the  keyword  *CON-
STRAINED_EULER_TO_EULER. 
•  Up  to  ten  ALE  multi-material  groups  may  now  be  defined.    The  previous  limit 
was three groups. 
•  Volume  fractions  can  be  automatically  assigned  during  initialization  of  multi-
material cells.  See the GEOMETRY option of *INITIAL_VOLUME_FRACTION. 
•  A new ALE smoothing option is available to accurately predict shock fronts. 
•  DATABASE_FSI activates output of fluid-structure interaction data to ASCII file 
DBFSI. 
•  Point sources for airbag inflators are available.  The origin and mass flow vector 
of these inflators are permitted to vary with time. 
•  A  majority  of  the  material  models  for  solid  materials  are  available  for  calcula-
tions using the SPH (Smooth Particle Hydrodynamics) option.   
•  The  Element  Free  Galerkin  method  (EFG  or  meshfree)  is  available  for  two-
dimensional and three-dimensional solids.  This new capability is not yet imple-
mented for MPP applications. 
•  A  binary  option  for  the  ASCII  files  is  now  available.    This  option  applies  to  all 
ASCII files and results in one binary file that contains all the information normal-
ly spread between a large number of separate ASCII files. 
•  Material models can now be defined by numbers rather than long names in the 
keyword  input.    For  example  the  keyword  *MAT_PIECEWISE_LINEAR_PLAS-
TICITY can be replaced by the keyword: *MAT_024. 
•  An  embedded  NASTRAN  reader  for  direct  reading  of  NASTRAN  input  files  is 
available.  This option allows a typical input file for NASTRAN to be read direct-
ly and used without additional input.  See the *INCLUDE_NASTRAN keyword.
History of LS-DYNA 
LS-DYNA Theory Manual 
•  Names in the keyword input can represent numbers if the *PARAMETER option 
is used to relate the names and the corresponding numbers.  
•  Model  documentation  for  the  major  ASCII  output  files  is  now  optional.    This 
option allows descriptors to be included within the ASCII files that document the 
contents of the file. 
•  ID’s have been added to the following keywords: 
◦  *BOUNDARY_PRESCRIBED_MOTION 
◦  *BOUNDARY_PRESCRIBED_SPC 
◦  *CONSTRAINED_GENERALIZED_WELD 
◦  *CONSTRAINED_JOINT 
◦  *CONSTRAINED_NODE_SET 
◦  *CONSTRAINED_RIVET 
◦  *CONSTRAINED_SPOTWELD 
◦  *DATABASE_CROSS_SECTION 
◦  *ELEMENT_MASS 
•  The  *DATABASE_ADAMS  keyword  is  available  to  output  a  modal  neutral  file 
d3mnf.    This  is  available  upon  customer  request  since  it  requires  linking  to  an 
ADAMS library file. 
•  Penetration  warnings  for  the  contact  option,  “ignore  initial  penetration,”  are 
added as an option.  Previously, no penetration warnings were written when this 
contact option was activated. 
•  Penetration  warnings  for  nodes  in-plane  with  shell  mid-surface  are  printed  for 
the AUTOMATIC contact options.  Previously, these nodes were ignored since it 
was assumed that they belonged to a tied interface where an offset was not used; 
consequently, they should not be treated in contact. 
•  For  the  arbitrary  spot  weld  option,  the  spot  welded  nodes  and  their  contact 
segments  are  optionally  written  into  the  d3hsp  file.    See  *CONTROL_CON-
TACT. 
•  For  the  arbitrary  spot  weld  option,  if  a  segment  cannot  be  found  for  the  spot 
welded  node,  an  option  now  exists  to  error  terminate.    See  *CONTROL_CON-
TACT. 
•  Spot weld resultant forces are written into the swforc file for solid elements used 
as spot welds. 
•  Solid materials have now been added to the failed element report and additional 
information is written for the “node is deleted” messages. 
•  A  new  option  for  terminating  a  calculation  is  available,  *TERMINATION_-
CURVE.
LS-DYNA Theory Manual 
History of LS-DYNA 
•  A  10-noded  tetrahedron  solid  element  is  available  with  either  a  4  or  5  point 
integration rule.  This element can also be used for implicit solutions. 
•  A  new  4  node  linear  shell  element  is  available  that  is  based  on  Wilson’s  plate 
element combined with a  Pian-Sumihara membrane element.   This is  shell type 
21. 
•  A shear panel element has been added for linear applications.  This is shell type 
22.  This element can also be used for implicit solutions. 
•  A  null  beam  element  for  visualization  is  available.    The  keyword  to  define  this 
null  beam  is  *ELEMENT_PLOTEL.    This  element  is  necessary  for  compatibility 
with NASTRAN. 
•  A  scalar  node  can  be  defined  for  spring-mass  systems.    The  keyword  to  define 
this node is *NODE_SCALAR.  This node can have from 1 to 6 scalar degrees-of-
freedom. 
•  A  thermal  shell  has  been  added  for  through-thickness  heat  conduction.  
Internally,  8  additional  nodes  are  created,  four  above  and  four  below  the  mid-
surface of the shell element.  A quadratic temperature field is modeled through 
the shell thickness.  Internally, the thermal shell is a 12 node solid element. 
•  A  beam  OFFSET  option  is  available  for  the  *ELEMENT_BEAM  definition  to 
permit  the  beam  to  be  offset  from  its  defining  nodal  points.    This  has  the  ad-
vantage that all beam formulations can now be used as shell stiffeners. 
•  A beam ORIENTATION option for orienting the beams by a vector instead of the 
third  node  is  available  in  the  *ELEMENT_BEAM  definition  for  NASTRAN 
compatibility.   
•  Non-structural  mass  has  been  added  to  beam  elements  for  modeling  trim  mass 
and for NASTRAN compatibility. 
•  An  optional  checking  of  shell  elements  to  avoid  abnormal  terminations  is 
available.  See *CONTROL_SHELL.  If this option is active, every shell is checked 
each  time  step  to  see  if  the  distortion  is  so  large  that  the  element  will  invert, 
which will result in an abnormal termination.  If a bad shell is detected, either the 
shell will be deleted or the calculation will terminate.  The latter is controlled by 
the input. 
•  An  offset  option  is  added  to  the  inertia  definition.    See  *ELEMENT_INERTIA_-
OFFSET  keyword.    This  allows  the  inertia  tensor  to  be  offset  from  the  nodal 
point. 
•  Plastic  strain  and  thickness  initialization  is  added  to  the  draw  bead  contact 
option.  See *CONTACT_DRAWBEAD_INITIALIZE. 
•  Tied contact with offsets based on both constraint equations and beam elements 
for  solid  elements  and  shell  elements  that  have  3  and  6  degrees-of-freedom  per 
node,  respectively.    See  BEAM_OFFSET  and  CONSTRAINED_OFFSET  contact 
options.  These options will not cause problems for rigid body motions.
History of LS-DYNA 
LS-DYNA Theory Manual 
•  The  segment-based  (SOFT =  2)  contact  is  implemented  for  MPP  calculations.  
This enables airbags to be easily deployed on the MPP version. 
•  Improvements  are  made  to  segment-based  contact  for  edge-to-edge  and  sliding 
conditions, and for contact conditions involving warped segments. 
•  An  improved  interior  contact  has  been  implemented  to  handle  large  shear 
deformations in the solid elements.  A special interior contact algorithm is avail-
able for tetrahedron elements. 
•  Coupling with MADYMO 6.0 uses an extended coupling that allows users to link 
most  MADYMO  geometric  entities  with  LS-DYNA  FEM  simulations.    In  this 
coupling  MADYMO  contact  algorithms  are  used  to  calculate  interface  forces 
between the two models. 
•  Release  flags  for  degrees-of-freedom  for  nodal  points  within  nodal  rigid  bodies 
are available.  This makes the nodal rigid body option nearly compatible with the 
RBE2 option in NASTRAN. 
•  Fast  updates  of  rigid  bodies  for  metal  forming  applications  can  now  be 
accomplished  by  ignoring  the  rotational  degrees-of-freedom  in  the  rigid  bodies 
that  are  typically  inactive  during  sheet  metal  stamping  simulations.    See  the 
keyword: *CONTROL_RIGID. 
•  Center  of  mass  constraints  can  be  imposed  on  nodal  rigid  bodies  with  the  SPC 
option in either a local or a global coordinate system. 
•  Joint failure based on resultant forces and moments can now be used to simulate 
the failure of joints. 
•  CONSTRAINED_JOINT_STIFFNESS  now  has  a  TRANSLATIONAL  option  for 
the translational and cylindrical joints. 
•  Joint  friction  has  been  added  using  table  look-up  so  that  the  frictional  moment 
can now be a function of the resultant translational force. 
•  The  nodal  constraint  options  *CONSTRAINED_INTERPOLATION  and  *CON-
STRAINED_LINEAR  now  have  a  local  option  to  allow  these  constraints  to  be 
applied in a local coordinate system. 
•  Mesh  coarsening  can  now  be  applied  to  automotive  crash  models  at  the 
beginning  of  an  analysis  to  reduce  computation  times.    See  the  new  keyword: 
*CONTROL_COARSEN. 
•  Force versus time seatbelt pretensioner option has been added. 
•  Both  static  and  dynamic  coefficients  of  friction  are  available  for  seat  belt  slip 
rings.  Previously, only one friction constant could be defined. 
•  *MAT_SPOTWELD now includes a new failure model with rate effects as well as 
additional failure options. 
•  Constitutive models added for the discrete beam elements:
LS-DYNA Theory Manual 
History of LS-DYNA 
◦  *MAT_1DOF_GENERALIZED_SPRING 
◦  *MAT_GENERAL_NONLINEAR_6dof_DISCRETE_BEAM  
◦  *MAT_GENERAL_NONLINEAR_1dof_DISCRETE_BEAM  
◦  *MAT_GENERAL_SPRING_DISCRETE_BEAM 
◦  *MAT_GENERAL_JOINT_DISCRETE_BEAM 
◦  *MAT_SEISMIC_ISOLATOR 
•  for shell and solid elements: 
◦  *MAT_PLASTICITY_WITH_DAMAGE_ORTHO 
◦  *MAT_SIMPLIFIED_JOHNSON_COOK_ORTHOTROPIC_DAMAGE 
◦  *MAT_HILL_3R  
◦  *MAT_GURSON_RCDC 
•  for the solid elements: 
◦  *MAT_SPOTWELD 
◦  *MAT_HILL_FOAM 
◦  *MAT_WOOD 
◦  *MAT_VISCOELASTIC_HILL_FOAM 
◦  *MAT_LOW_DENSITY_SYNTHETIC_FOAM 
◦  *MAT_RATE_SENSITIVE_POLYMER 
◦  *MAT_QUASILINEAR VISCOELASTIC 
◦  *MAT_TRANSVERSELY_ANISOTROPIC_CRUSHABLE_FOAM 
◦  *MAT_VACUUM  
◦  *MAT_MODIFIED_CRUSHABLE_FOAM 
◦  *MAT_PITZER_CRUSHABLE FOAM 
◦  *MAT_JOINTED_ROCK 
◦  *MAT_SIMPLIFIED_RUBBER 
◦  *MAT_FHWA_SOIL 
◦  *MAT_SCHWER_MURRAY_CAP_MODEL 
•  Failure time added to MAT_EROSION for solid elements. 
•  Damping  in  the  material  models  *MAT_LOW_DENSITY_FOAM  and  *MAT_-
LOW_DENSITY_VISCOUS_FOAM  can  now  be  a  tabulated  function  of  the 
smallest stretch ratio. 
•  The  material  model  *MAT_PLASTICITY_WITH_DAMAGE  allows  the  table 
definitions for strain rate.
History of LS-DYNA 
LS-DYNA Theory Manual 
•  Improvements in the option *INCLUDE_STAMPED_PART now allow all history 
data  to  be  mapped  to  the  crash  part  from  the  stamped  part.    Also,  symmetry 
planes can be used to allow the use of a single stamping to initialize symmetric 
parts. 
•  Extensive  improvements  in  trimming  result  in  much  better  elements  after  the 
trimming is completed.  Also, trimming can be defined in either a local or global 
coordinate system.  This is a new option in *DEFINE_CURVE_TRIM. 
•  An option to move parts close before solving the contact problem is available, see 
*CONTACT_AUTO_MOVE.  
•  An option to add or remove discrete beams during a calculation is available with 
the new keyword: *PART_SENSOR. 
•  Multiple  jetting  is  now  available  for  the  Hybrid  and  Chemkin  airbag  inflator 
models. 
•  Nearly all constraint types are now handled for implicit solutions. 
•  Calculation of constraint and attachment modes can be easily done by using the 
option: *CONTROL_IMPLICIT_MODES. 
•  Penalty  option,  see  *CONTROL_CONTACT,  now  applies  to  all  *RIGIDWALL 
options and is always used when solving implicit problems. 
•  Solid  elements  types  3  and  4,  the  4  and  8  node  elements  with  6  degrees-of-
freedom per node, are available for implicit solutions. 
•  The  warping  stiffness  option  for  the  Belytschko-Tsay  shell  is  implemented  for 
implicit  solutions.    The  Belytschko-Wong-Chang  shell  element  is  now  available 
for  implicit  applications.    The  full  projection  method  is  implemented  due  to  it 
accuracy over the drill projection. 
•  Rigid to deformable switching is implemented for implicit solutions. 
•  Automatic  switching  can  be  used  to  switch  between  implicit  and  explicit 
calculations.  See the keyword: *CONTROL_IMPLICIT_GENERAL. 
•  Implicit dynamics rigid bodies are now implemented.  See the keyword  *CON-
TROL_IMPLICIT_DYNAMIC. 
•  Eigenvalue solutions can be intermittently calculated during a transient analysis. 
•  A  linear  buckling  option  is  implemented.    See  the  new  control  input:  *CON-
TROL_IMPLICIT_BUCKLE 
•  Implicit  initialization  can  be  used  instead  of  dynamic  relaxation.    See  the 
keyword *CONTROL_DYNAMIC_RELAXATION where the parameter, IDFLG, 
is set to 5. 
•  Superelements,  i.e.,  *ELEMENT_DIRECT_MATRIX_INPUT,  are  now  available 
for implicit applications.
LS-DYNA Theory Manual 
History of LS-DYNA 
•  There is an extension of the option, *BOUNDARY_CYCLIC, to symmetry planes 
in  the  global  Cartesian  system.    Also,  automatic  sorting  of  nodes  on  symmetry 
planes is now done by LS-DYNA. 
•  Modeling  of  wheel-rail  contact  for  railway  applications  is  now  available,  see 
*RAIL_TRACK and *RAIL_TRAIN. 
•  A  new,  reduced  CPU,  element  formulation  is  available  for  vibration  studies 
when elements are aligned with the global coordinate system.  See *SECTION_-
SOLID and *SECTION_SHELL formulation 98. 
•  An option to provide approximately constant damping over a range of frequen-
cies is implemented, see *DAMPING_FREQUENCY_RANGE.
LS-DYNA Theory Manual 
Preliminaries 
3    
Preliminaries 
NOTE: Einstein summation convention is used.  For each re-
peated index there is an implied summation. 
Consider  the  body  shown  in  Figure  3.1.    We  are  interested  in  time-dependent 
deformation  for  which  a  point  in  b  initially  at  𝑋𝛼  (𝛼 = 1,  2,  3)  in  a  fixed  rectangular 
Cartesian  coordinate  system  moves  to  a  point  𝑥𝑖  (𝑖 = 1,  2,  3)  in  the  same  coordinate 
system.    Since  a  Lagrangian  formulation  is  considered,  the  deformation  can  be 
expressed in terms of the convected coordinates 𝑋𝛼, and time 𝑡 
At time 𝑡 = 0, we have the initial conditions 
𝑥𝑖 = 𝑥𝑖(𝑋𝛼, 𝑡).
𝑥𝑖(𝐗, 0) = 𝑋i
𝑥̇𝑖(𝐗, 0) = 𝑉𝑖(𝐗)
where 𝐕 is the initial velocity. 
3.1  Governing Equations 
We seek a solution to the momentum equation 
𝜎𝑖𝑗,𝑗 + 𝜌𝑓𝑖 = 𝜌𝑥̈𝑖
satisfying the traction boundary conditions,  
𝜎𝑖𝑗𝑛𝑗 = 𝑡𝑖(𝑡),
on boundary 𝜕𝑏1, the displacement boundary conditions, 
𝑥𝑖(𝑋𝛼, 𝑡) = 𝐷𝑖(𝑡),
on boundary 𝜕𝑏2, and the contact discontinuity condition, 
(𝜎𝑖𝑗
+ − 𝜎𝑖𝑗
−)𝑛𝑖 = 0,
(3.1)
(3.2)
(3.3)
(3.4)
(3.5)
(3.6)
Preliminaries 
LS-DYNA Theory Manual 
 + = 𝑥𝑖
 −.    Here  𝛔  is  the  Cauchy  stress,  𝜌  is  the 
along  an  interior  boundary  𝜕b3  when  𝑥𝑖
current  density,  𝐟  is  the  body  force  density,  and  𝐱̈  is  acceleration.    The  comma  on  𝜎𝑖𝑗,𝑗 
denotes  covariant  differentiation,  and  𝑛𝑗  is  a  unit  outward  normal  to  a  boundary 
element on ∂b. 
Mass conservation is trivially stated as 
where 𝑉 is the relative volume, i.e., the determinant of the deformation gradient matrix, 
𝐹𝑖𝑗, 
𝜌𝑉 = 𝜌0
(3.7)
𝐹𝑖𝑗 =
∂𝑥𝑖
∂𝑋𝑗
and 𝜌0 is the reference density.  The energy equation 
𝐸̇ = 𝑉𝑠𝑖𝑗𝜀̇𝑖𝑗 − (𝑝 + 𝑞)𝑉̇
(3.8)
(3.9)
is integrated in time and is used for evaluating equations of state and to track the global 
energy  balance.    In  Equation  (3.9),  𝑠𝑖𝑗  and  𝑝  represent  the  deviatoric  stresses  and 
pressure, 
𝑠𝑖𝑗 = 𝜎𝑖𝑗 + (𝑝 + 𝑞)𝛿𝑖𝑗
𝑝 = −
= −
𝜎𝑖𝑗𝛿𝑖𝑗 − 𝑞 
𝜎𝑘𝑘 − 𝑞
(3.10)
(3.11)
respectively,  where  𝑞  is  the  bulk  viscosity,  𝛿𝑖𝑗  is  the  Kronecker  delta  (𝛿𝑖𝑗 = 1  if  𝑖 = 𝑗; 
otherwise 𝛿𝑖𝑗 = 0), and 𝜀̇𝑖𝑗 is the strain rate tensor.  The strain rates and bulk viscosity are 
discussed later.
LS-DYNA Theory Manual 
Preliminaries 
X3
x3
x2
X2
∂
t = 0
B0
∂
X1
x1
Figure 3.1.  Notation. 
We can write: 
∫ (𝜌𝑥̈𝑖 − 𝜎𝑖𝑗,𝑗 − 𝜌𝑓 )𝛿𝑥𝑖𝑑𝜐 + ∫ (𝜎𝑖𝑗𝑛𝑗 − 𝑡𝑖)𝛿𝑥𝑖𝑑𝑠
𝜕𝑏1
+ ∫ (𝜎𝑖𝑗
𝜕𝑏3
+ − 𝜎𝑖𝑗
−)𝑛𝑗𝛿𝑥𝑖𝑑𝑠 = 0
(3.12)
where  𝛿𝑥𝑖  satisfies  all  boundary  conditions  on  𝜕𝑏2,  and  the  integrations  are  over  the 
current geometry.  Application of the divergence theorem gives 
∫ (𝜎𝑖𝑗𝛿𝑥𝑖)
,𝑗
 𝑑𝜐
= ∫ 𝜎𝑖𝑗𝑛𝑗𝛿𝑥𝑖𝑑𝑠
∂𝑏1
and noting that 
+ ∫ (𝜎𝑖𝑗
∂𝑏3
+ − 𝜎𝑖𝑗
−)𝑛𝑗𝛿𝑥𝑖𝑑𝑠
leads to the weak form of the equilibrium equation, 
(𝜎𝑖𝑗𝛿𝑥𝑖),𝑗− 𝜎𝑖𝑗,𝑗𝛿𝑥𝑖 = 𝜎𝑖𝑗𝛿𝑥𝑖,𝑗
𝛿𝜋 = ∫ 𝜌𝑥̈𝑖𝛿𝑥𝑖𝑑𝜐
+ ∫ 𝜎𝑖𝑗𝛿𝑥𝑖,𝑗𝑑𝜐
− ∫ 𝜌𝑓𝑖𝛿𝑥𝑖𝑑𝜐
− ∫ 𝑡𝑖𝛿𝑥𝑖𝑑𝑠
∂𝑏1
= 0, 
which is a statement of the principle of virtual work. 
(3.13)
(3.14)
(3.15)
We superimpose a mesh of finite elements interconnected at nodal points on the 
reference configuration and track particles through time, i.e., 
𝑥𝑖(𝑋𝛼, 𝑡) = 𝑥𝑖(𝑋𝛼(𝜉 , 𝜂, 𝜁 ), 𝑡) = ∑ 𝑁𝑗(𝜉 , 𝜂, 𝜁 )𝑥𝑖
 𝑗(𝑡)
(3.16)
𝑗=1
Preliminaries 
LS-DYNA Theory Manual 
where 𝑁𝑗 are shape (interpolation) functions in the parametric coordinates (𝜉 , 𝜂, 𝜁 ), 𝑘 is 
 𝑗 is the nodal coordinate of the jth 
the number of nodal points defining the element, and 𝑥𝑖
node in the ith direction.  Each shape function has a finite support that is limited to the 
elements  for  which  its  associated  node  is  a  member  (hence  the  name  finite  element 
method).    Consequently,  within  each  element  the  interpolation  only  depends  on  the 
nodal  values  for  the  nodes  in  that  element,  and  hence  expressions  like  Equation 
(3.16)are meaningful. 
The condition 𝛿𝜋 = 0 holds for all variations, 𝛿𝑥𝑖, and, in particular, it holds for 
variations along the shape functions.  In each of the 3 Cartesian directions upon setting 
the  variation  to  one  of  the  shape  functions  the  weak  form  reduces  to  a  necessary  (but 
not sufficient) condition that must be satisfied by any solution so that the 
number of equations = 3 × number of nodes. 
At this stage it is useful to introduce a vector space having dimension ℝ(number of nodes) 
number of nodes.  Since the body is discretized into 
with a corresponding cartesian basis {𝐞𝑖
𝑛 disjoint elements, the integral in (3.15) may be separated using the spatial additively 
of integration into 𝑛 terms, one for each element 
′}𝑖=1
𝛿𝜋 = ∑ 𝛿𝜋𝑚 = 0
.
𝑚=1
The contribution from each element is 
𝛿𝜋𝑚 = ∫ 𝜌𝑥̈𝑖𝛿𝑥𝑖𝑑𝜐
𝜐𝑚
+ ∫ 𝜎𝑖𝑗𝛿𝑥𝑖,𝑗𝑑𝜐
𝜐𝑚
− ∫ 𝜌𝑓𝑖𝛿𝑥𝑖𝑑𝜐
𝜐𝑚
− ∫
∂𝑏1∩𝜕𝑣𝑚
𝑡𝑖𝛿𝑥𝑖𝑑𝑠
. 
Assembling the element contributions back into a system of equations leads to 
∑ {∫ 𝜌𝑥̈𝑖(𝐞i⨂𝛎𝑚)𝑑𝜐 +
𝑚=1
𝜐𝑚
𝑚(𝐞i⨂𝛎,𝑗
𝑚)𝑑𝜐
∫ 𝜎𝑖𝑗
𝜐𝑚
− ∫ 𝜌𝑓𝑖(𝐞i⨂𝛎𝑚)𝑑𝜐
𝜐𝑚
− ∫
∂𝑏1∩𝜕𝑣𝑚
𝑡𝑖(𝐞i⨂𝛎𝑚)𝑑𝑠
} = 0. 
In which 
𝛎𝑚 = ∑ 𝑁𝑖𝐞𝑛𝑚(𝑖)
′
(3.17)
(3.18)
(3.19)
(3.20)
where 𝑛𝑚(𝑖) is the global node number. 
𝑖=1
Applying  the  approximation  scheme  of  Equation  (3.16)  to  the  dependent 
variables and substituting into Equation (3.19) yields 
∑ {∫ 𝜌𝐍𝑚
𝜐𝑚
𝑚=1
T 𝐍𝑚𝐚𝑑𝜐
+ ∫ 𝐁𝑚
𝜐𝑚
T 𝛔𝑑𝜐
− ∫ 𝜌𝐍𝑚
𝜐𝑚
T 𝐛𝑑𝜐
− ∫ 𝐍𝑚
∂𝑏1
T 𝐭𝑑𝑠
}
= 0 
where 𝐍 is an interpolation matrix; 𝜎 is the stress vector 
𝛔T = (𝜎𝑥𝑥, 𝜎𝑦𝑦, 𝜎𝑧𝑧, 𝜎𝑥𝑦, 𝜎𝑦𝑧, 𝜎zx);
(3.21)
(3.22)
LS-DYNA Theory Manual 
Preliminaries 
B is the strain-displacement matrix; a is the nodal acceleration vector 
𝑥̈1
⎤ = 𝐍
⎡
𝑥̈2
⎥
⎢
𝑥̈3⎦
⎣
𝑎𝑥
⎤
⎡
⎥
⎢
𝑎𝑥
⎥
⎢
⋮
⎥
⎢
⎥
⎢
𝑎𝑦
⎥
⎢
𝑘⎦
𝑎𝑧
⎣
= 𝐍𝐚; 
(3.23)
b is the body force load vector; and 𝒕 is the applied traction load. 
𝐛 =
𝑓𝑥
⎤
⎡
𝑓𝑦
⎥⎥
⎢⎢
𝑓𝑧⎦
⎣
,     𝐭 =
𝑡𝑥
⎤
⎡
𝑡𝑦
⎥
⎢
𝑡𝑧⎦
⎣
(3.24)
LS-DYNA Theory Manual 
Solid Elements 
4    
Solid Elements 
For a mesh of 8-node hexahedron solid elements, Equation ((3.16)) becomes: 
𝑥𝑖(𝑋𝛼, 𝑡) = 𝑥𝑖(𝑋𝛼(𝜉 , 𝜂, 𝜁 ), 𝑡) = ∑ 𝜙𝑗(𝜉 , 𝜂, 𝜁 )𝑥𝑖
 𝑗(𝑡)
.
The shape function 𝜙𝑗 is defined for the 8-node hexahedron as 
𝑗=1
𝜙𝑗 =
(1 + 𝜉 𝜉𝑗)(1 + 𝜂𝜂𝑗)(1 + 𝜁 𝜁𝑗),
(4.1)
(4.2)
where 𝜉𝑗, 𝜂𝑗, 𝜁𝑗 take on their nodal values of (±1, ±1, ±1) and 𝑥𝑖
the jth node in the ith direction . 
𝑗 is the nodal coordinate of 
For a solid element, N is the 3 × 24 rectangular interpolation matrix given by 
N(𝜉 , 𝜂, 𝜁 ) =
𝜙1
⎡
⎢
⎣
𝜙1
𝜙1
𝜙2
0 ⋯ 0
𝜙2 ⋯ 𝜙8
0 ⋯ 0
⎤
, 
⎥
𝜙8⎦
𝝈 is the stress vector 
σT = (𝜎𝑥𝑥 𝜎𝑦𝑦 𝜎𝑧𝑧 𝜎𝑥𝑦 𝜎𝑦𝑧 𝜎𝑧𝑥).
(4.3)
(4.4)
Solid Elements 
LS-DYNA Theory Manual 
Node
-1
-1
-1
-1
-1
-1
-1
-1
-1
-1
-1
-1
Figure 4.1.  Eight node solid hexahedron element. 
𝐁 is the 6 × 24 strain-displacement matrix 
𝐁 =
∂
∂𝑥
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
∂
∂𝑦
∂
∂𝑧
∂
∂𝑦
∂
∂𝑥
∂
∂𝑧
∂
∂𝑧
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
∂
⎥
⎥
∂𝑦
⎥
∂
⎥
∂𝑥⎦
𝐍. 
(4.5)
In order to achieve a diagonal mass matrix the rows are summed giving the kth diagonal 
term as 
𝑚𝑘𝑘 = ∫ 𝜌𝜙𝑘 ∑ 𝜙𝑖𝑑𝜐 = ∫ 𝜌𝜙𝑘𝑑𝜐
,
(4.6)
𝑖=1
since the basis functions sum to unity. 
Terms in the strain-displacement matrix are readily calculated.  Note that
LS-DYNA Theory Manual 
Solid Elements 
∂𝜙𝑖
∂𝜉
∂𝜙𝑖
∂𝜂
∂𝜙𝑖
∂𝜁
=
=
=
∂𝜙𝑖
∂𝑥
∂𝜙𝑖
∂𝑥
∂𝜙𝑖
∂𝑥
∂𝑥
∂𝜉
∂𝑥
∂𝜂
∂𝑥
∂𝜁
+
+
+
∂𝜙𝑖
∂𝑦
∂𝜙𝑖
∂𝑦
∂𝜙𝑖
∂𝑦
∂𝑦
∂𝜉
∂𝑦
∂𝜂
∂𝑦
∂𝜁
+
+
+
∂𝜙𝑖
∂𝑧
∂𝜙𝑖
∂𝑧
∂𝜙𝑖
∂𝑧
∂𝑧
∂𝜉
∂𝑧
∂𝜂
∂𝑧
∂𝜁
, 
, 
, 
which can be rewritten as 
∂𝜙𝑖
⎤
⎡
∂𝜉
⎥
⎢
⎥
⎢
∂𝜙𝑖
⎥
⎢
⎥
⎢
∂𝜂
⎥
⎢
⎥
⎢
∂𝜙𝑖
⎥
⎢
∂𝜁 ⎦
⎣
=
∂𝑥
∂𝜉
∂𝑥
∂𝜂
∂𝑥
∂𝜁
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
∂𝑦
∂𝜉
∂𝑦
∂𝜂
∂𝑦
∂𝜁
∂𝑧
⎤
∂𝜉
⎥
⎥
∂𝑧
⎥
⎥
∂𝜂
⎥
⎥
∂𝑧
⎥
∂𝜁 ⎦
∂𝜙𝑖
⎤
⎡
∂𝑥
⎥
⎢
⎥
⎢
∂𝜙𝑖
⎥
⎢
⎥
⎢
∂𝑦
⎥
⎢
∂𝜙𝑖
⎥
⎢
∂𝑧 ⎦
⎣
= 𝐉
∂𝜙𝑖
⎤
⎡
∂𝑥
⎥
⎢
⎥
⎢
∂𝜙𝑖
⎥
⎢
. 
⎥
⎢
∂𝑦
⎥
⎢
∂𝜙𝑖
⎥
⎢
∂𝑧 ⎦
⎣
Inverting the Jacobian matrix, J, we can solve for the desired terms 
∂𝜙𝑖
⎤
⎡
∂𝑥
⎥
⎢
⎥
⎢
∂𝜙𝑖
⎥
⎢
⎥
⎢
∂𝑦
⎥
⎢
∂𝜙𝑖
⎥
⎢
∂𝑧 ⎦
⎣
= 𝐉−1
∂𝜙𝑖
⎤
⎡
∂𝜉
⎥
⎢
⎥
⎢
∂𝜙𝑖
⎥
⎢
⎥
⎢
∂𝜂
⎥
⎢
⎥
⎢
∂𝜙𝑖
⎥
⎢
∂𝜁 ⎦
⎣
. 
(4.7)
(4.8)
(4.9)
4.1  Volume Integration 
Volume  integration  is  carried  out  with  Gaussian  quadrature.    If  𝑔  is  some 
function defined over the volume, and 𝑛 is the number of integration points, then 
∫ 𝑔𝑑𝜐 = ∫ ∫ ∫ 𝑔|𝐉|𝑑𝜉𝑑𝜂𝑑𝜁
−1
−1
−1
,
is approximated by 
∑ ∑ ∑ 𝑔𝑗𝑘𝑙∣𝐽𝑗𝑘𝑙∣𝑤𝑗𝑤𝑘𝑤𝑙
𝑗=1
𝑘=1
𝑙=1
,
where 𝑤𝑗, 𝑤𝑘, 𝑤𝑙 are the weighting factors, 
𝑔𝑗𝑘𝑙 = g(𝜉𝑗, 𝜂𝑘, 𝜁𝑙),
and 𝐽 is the determinant of the Jacobian matrix.  For one-point quadrature 
𝑛 = 1,
𝑤𝑖 = 𝑤𝑗 = 𝑤𝑘 = 2,
(4.10)
(4.11)
(4.12)
(4.13)
Solid Elements 
LS-DYNA Theory Manual 
Strain displacement matrix
Strain rates
Force
Subtotal
Hourglass control
Total
DYNA3D 
Flanagan 
Belytschko 
Wilkins 
FDM 
94 
87 
117 
298 
130 
428 
357 
156 
195 
708 
620 
1328 
843 
270 
1113 
680 
1793 
Table 4.1.   Operation counts  for a constant stress  hexahedron (includes adds,
subtracts, multiplies, and divides in major subroutines, and is independent of
vectorization).  Material subroutines will add as little as 60 operations for the
bilinear elastic-plastic routine to ten times as much for multi-surface plasticity 
and  reactive  flow  models.    Unvectorized  material  models  will  increase  that
share of the cost a factor of four or more. 
and we can write 
𝜉1 = 𝜂1 = 𝜁1 = 0,
Note that 8|𝐽(0,0,0)| approximates the element volume. 
∫ 𝑔𝑑𝑣 = 8𝑔(0,0,0)|𝐉(0,0,0)|.
(4.14)
Perhaps the biggest advantage to one-point integration is a substantial savings in 
computer time.  An anti-symmetry property of the strain matrix 
,
,
,
= −
= −
= −
= −
∂𝜙7
∂𝑥𝑖
∂𝜙8
∂𝑥𝑖
∂𝜙1
∂𝑥𝑖
∂𝜙2
∂𝑥𝑖
∂𝜙5
∂𝑥𝑖
∂𝜙6
∂𝑥𝑖
∂𝜙3
∂𝑥𝑖
∂𝜙4
∂𝑥𝑖
at 𝜉 = 𝜂 = 𝜁 = 0 reduces the amount of effort required to compute this matrix by more 
than  25  times  over  an  8-point  integration.    This  cost  savings  extends  to  strain  and 
element nodal force calculations where the number of multiplies is reduced by a factor 
of 16.  Because only one constitutive evaluation is needed, the time spent determining 
stresses is reduced by a factor of 8.  Operation counts for the constant stress hexahedron 
are  given  in  Table  4.1.    Included  are  counts  for  the  Flanagan  and  Belytschko  [1981] 
hexahedron and the hexahedron used by Wilkins [1974] in his integral finite difference 
method, which was also implemented [Hallquist 1979].  
,
(4.15)
It may be noted that 8-point integration has another disadvantage in addition to 
cost.    Fully  integrated  elements  used  in  the  solution  of  plasticity  problems  and  other
LS-DYNA Theory Manual 
Solid Elements 
problems where Poisson’s ratio approaches 0.5 lock up in the constant volume bending 
modes.    To  preclude  locking,  an  average  pressure  must  be  used  over  the  elements; 
consequently,  the  zero  energy  modes  are  resisted  by  the  deviatoric  stresses.    if  the 
deviatoric stresses are insignificant relative to the pressure or,  even worse, if material 
failure cause loss of this stress state component, hourglassing will  still occur, but with 
no means of resisting it.  Sometimes, however, the cost of the fully integrated element 
may be justified by increased reliability and if used sparingly may actually increase the 
overall speed.
4.2  Solid Element 2 
Solid  element  2  is  a  selective  reduced  (S/R)  integrated  element  that  in  general  is 
regarded as too stiff.  In particular this is the case when the elements exhibit poor aspect 
ratio,  i.e.,  when  one  element  dimension  is  significantly  smaller than  the  other(s).    This 
occurs for instance when modelling thin walled structures and the time for solving the 
problem prevents using a sufficient number of elements for maintaining close to cubic 
elements throughout the structure.  The reason for the locking phenomenon is that the 
element  is  not  able  to  represent  pure  bending  modes  without  introducing  transverse 
shear strains, and this may be bad enough to lock the element to a great extent.  In an 
attempt to  solve  this  transverse  shear  locking  problem, two  new  fully  integrated  solid 
elements  are  introduced  and  documented  herein  that  may  become  of  practical  use  for 
these types of applications. 
4.2.1  Brief summary of solid element 2 
Let  𝑥𝐼𝑖  represent  the  nodal  coordinate  of  dimension  𝑖  and  node  𝐼,  and  likewise  𝑣𝐼𝑖  its 
velocity.  Furthermore denote 
𝑁𝐼(𝜉1, 𝜉2, 𝜉3) =
(1 + 𝜉1
𝐼𝜉1 + 𝜉2
𝐼𝜉2 + 𝜉3
𝐼𝜉3 + 𝜉12
𝐼 𝜉1𝜉2 + 𝜉13
𝐼 𝜉1𝜉3 + 𝜉23
𝐼 𝜉2𝜉3 + 𝜉123
𝐼 𝜉1𝜉2𝜉3),(4.2.16)
the shape functions for the standard isoparametric domain where 
1 −1 −1
∗ = [−1
𝜉1
∗ = [−1 −1
𝜉2
1 −1 −1
∗ = [−1 −1 −1 −1
𝜉3
∗ = [ 1 −1
𝜉12
1 −1
1 −1
∗ = [ 1 −1 −1
𝜉13
1 −1
∗ = [ 1
𝜉23
1 −1 −1 −1 −1
∗ = [−1
𝜉123
1 −1
1 −1
and let furthermore 
1 −1],
1], 
1], 
1 −1], 
1 −1], 
1], 
1 −1], 
𝐼 ,
𝐼 = 𝜉12
𝜉21
𝐼 = 𝜉23
𝐼 , 
𝜉32
𝐼 .
𝐼 = 𝜉13
𝜉31
(4.2.17)
(4.2.18)
Solid Elements 
LS-DYNA Theory Manual 
Figure 4.2.2.  Bending mode for a fully integrated brick. 
The  isoparametric  representation  of  the  coordinates  of  a  material  point  in  the 
element is then given as (where the dependence on 𝜉1, 𝜉2, 𝜉3 is suppressed for brevity) 
and its associated jacobian matrix is 
𝑥𝑖 = 𝑥𝐼𝑖𝑁𝐼,
𝐽𝑖𝑗 =
𝜕𝑥𝑖
𝜕𝜉𝑗
= 𝑥𝐼𝑖
(𝜉𝑗
𝐼 + 𝜉𝑗𝑘
𝐼 𝜉𝑘 + 𝜉𝑗𝑙
𝐼 𝜉𝑙 + 𝜉123
𝐼 𝜉𝑘𝜉𝑙),
(4.2.19)
(4.2.20)
where 𝑘 = 1 + mod(𝑗, 3) and 𝑙 = 1 + mod(𝑗 + 1,3). For future reference let 
be the jacobian evaluated in the element center and in the beginning of the simulation 
(i.e.,  at  time  zero).    The  velocity  gradient  computed  directly  from  the  shape  functions 
and velocity components is 
0 = 𝑥𝐼𝑖(0)
𝐽𝑖𝑗
(4.2.21)
𝐼,
𝜉𝑗
where 
𝐿𝑖𝑗 =
𝜕𝑣𝑖
𝜕𝑥𝑗
= 𝐽 ̇𝑖𝑘𝐽𝑘𝑗
−1 = 𝐵𝑖𝑗𝐼𝑘𝑣𝐼𝑘,
𝐵𝑖𝑗𝐼𝑘 =
𝜕𝑁𝐼
𝜕𝜉𝑙
−1𝛿𝑖𝑘,
𝐽𝑙𝑗
(4.2.22)
(4.2.23)
is  the  gradient-displacement  matrix  and  represents  the  element  except  for  the 
alleviation of volumetric locking.  To do just that, let 𝐵𝑖𝑗𝐼𝑘
0  be defined by 
0 𝑣𝐼𝑘,
with  𝐽 ̅𝑖𝑗  being  the  element  averaged  jacobian  matrix,  and  construct  the  gradient-
displacement matrix used for the element as 
−1 = 𝐵𝑖𝑗𝐼𝑘
𝑖𝑘𝐽 ̅
𝐽 ̅
𝑘𝑗
(4.2.24)
𝐵̅̅̅̅𝑖𝑗𝐼𝑘 = 𝐵𝑖𝑗𝐼𝑘 +
(𝐵𝑙𝑙𝐼𝑘
0 − 𝐵𝑙𝑙𝐼𝑘)𝛿𝑖𝑗.
(4.2.25)
This is what is often called the B-bar method. 
4-6 (Solid Elements)
LS-DYNA Theory Manual 
Solid Elements 
4.2.2  Transverse shear locking example 
To  get  the  idea  of  the  modifications  needed  to  alleviate  transverse  shear  locking  let’s 
look at the parallelepiped of dimensions 𝑙1 × 𝑙2 × 𝑙3 in the Figure above. For this simple 
geometry the jacobian matrix is diagonal and the velocity gradient is expressed as 
𝐿𝑖𝑗 =
𝑙𝑗
𝐽 ̇𝑖𝑗 =
4𝑙𝑗
𝑣𝐼𝑖(𝜉𝑗
𝐼 + 𝜉𝑗𝑘
𝐼 𝜉𝑘 + 𝜉𝑗𝑙
𝐼 𝜉𝑙 + 𝜉123
𝐼 𝜉𝑘𝜉𝑙),
(4.2.26)
where,  again,  𝑘 = 1 + mod(𝑗, 3)  and  𝑙 = 1 + mod(𝑗 + 1,3).  Now  let  𝑖 ≠ 𝑝 ≠ 𝑞 ≠ 𝑖,  then  a 
pure  bending  mode  in  the  plane  with  normal  in  direction  𝑞  and  about  axis  𝑝  is 
represented by 
𝐼 ,
𝑣𝐼𝑖 = 𝜉𝑖𝑞
𝑣𝐼𝑝 = 0, 
𝑣𝐼𝑞 = 0,
and thus the velocity gradient is given as 
(𝜉𝑖𝑞
𝐼 𝜉𝑗𝑘
𝐼 𝜉𝑘 + 𝜉𝑖𝑞
𝐼 𝜉𝑗𝑙
𝐼 𝜉𝑙),
𝐿𝑖𝑗 =
4𝑙𝑗
𝐿𝑝𝑗 = 0, 
𝐿𝑞𝑗 = 0,
for 𝑗 = 1, 2, 3.  The nonzero expression above amounts to 
𝐿𝑖𝑖 =
4𝑙𝑖
𝐿𝑖𝑝 = 0, 
4𝑙𝑞
𝐿𝑖𝑞 =
𝜉𝑞,
𝜉𝑖.
(4.2.27)
(4.2.28)
(4.2.29)
Notable  here  is  that  a  pure  bending  mode  gives  arise  to  a  transverse  shear  strain 
represented by the last expression in the above. Assuming that 𝑙𝑞 is small compared to 𝑙𝑖 
this may actually lock the element. 
4.2.3  Solid element -2 
Given  this  insight  the  modifications  in  the  expression  of  the  jacobian  matrix  are  as 
follows.  Let 
𝜅𝑚𝑛 = min
0 + 𝐽2𝑚
0 + 𝐽2𝑛
be the aspect ratio between dimensions 𝑚 and 𝑛 at time zero.  The modified jacobian is 
written 
0 + 𝐽3𝑚
0 + 𝐽3𝑛
0 𝐽3𝑚
0 𝐽3𝑛
0 𝐽1𝑚
0 𝐽1𝑛
0 𝐽2𝑚
0 𝐽2𝑛
√𝐽1𝑚
√𝐽1𝑛
⎜⎜⎜⎛
⎝
⎟⎟⎟⎞
⎠
(4.2.30)
1,
, 
𝐽 ̃𝑖𝑗 = 𝑥𝐼𝑖
where 
LS-DYNA Draft 
(𝜉𝑗
𝐼 + 𝜉𝑗𝑘
𝐼 𝜉𝑘𝑖 + 𝜉𝑗𝑙
𝐼 𝜉𝑙𝑖 + 𝜉123
𝐼 𝜉𝑘𝑖𝜉𝑙𝑖),
Solid Elements 
LS-DYNA Theory Manual 
and 
𝜉𝑘𝑖 = {
𝜉𝑘𝜅𝑗𝑘
𝜉𝑘
𝑖 ≠ 𝑗
otherwise
,
𝜉𝑙𝑖 = {
𝜉𝑙𝜅𝑗𝑙
𝜉𝑙
𝑖 ≠ 𝑗
otherwise
.
The velocity gradient is now given as 
(4.2.32)
(4.2.33)
−1 = 𝐵̃ 𝑖𝑗𝐼𝑘𝑣𝐼𝑘,
𝑖𝑘𝐽 ̃
𝑘𝑗
where  𝐵̃ 𝑖𝑗𝐼𝑘  is  the  gradient-displacement  matrix  used  for  solid  element  type  -2  in  LS-
DYNA. The B-bar method is used to prevent volumetric locking. 
𝐿𝑖𝑗 = 𝐽 ̃
(4.2.34)
4.2.4  Transverse shear locking example revisited 
Once again let’s look at the parallelepiped of dimensions 𝑙1 × 𝑙2 × 𝑙3. The jacobian matrix 
is  still  diagonal  and  the  velocity  gradient  is  with  the  new  element  formulation 
expressed as 
𝐿𝑖𝑗 =
𝑙𝑗
𝐽 ̃
𝑖𝑗 =
4𝑙𝑗
𝑣𝐼𝑖(𝜉𝑗
𝐼 + 𝜉𝑗𝑘
𝐼 𝜉𝑘𝑖 + 𝜉𝑗𝑙
𝐼 𝜉𝑙𝑖 + 𝜉123
𝐼 𝜉𝑘𝑖𝜉𝑙𝑖),
(4.2.35)
where,  again,  𝑘 = 1 + mod(𝑗, 3)  and  𝑙 = 1 + mod(𝑗 + 1,3).  The  velocity  gradient  for  a 
pure bending mode is now given as 
𝐿𝑖𝑗 =
4𝑙𝑗
(𝜉𝑖𝑞
𝐼 𝜉𝑗𝑘
𝐼 𝜉𝑘𝑖 + 𝜉𝑖𝑞
𝐼 𝜉𝑗𝑙
𝐼 𝜉𝑙𝑖),
which amounts to (for the potential nonzero elements) 
𝜉𝑞,
𝐿𝑖𝑖 =
4𝑙𝑖
𝐿𝑖𝑝 = 0, 
4𝑙𝑞
𝐿𝑖𝑞 =
𝜉𝑖𝜅𝑞𝑖. 
(4.2.36)
(4.2.37)
If we assume that this is the geometry in the beginning of the simulation and that 
𝑙𝑞 is smaller than 𝑙𝑖 the transverse shear strain can be expressed as 
meaning that the transverse shear energy is not affected by poor aspect ratios, i.e., the 
transverse shear strain does not grow with decreasing 𝑙𝑞. 
𝐿𝑖𝑞 =
4𝑙𝑖
𝜉𝑖, 
(4.2.38)
4.2.5  Solid element -1 
Working out the details in the expression of the gradient-displacement matrix for solid 
element type -2 reveals that this matrix is dense, i.e., there are 216 nonzero elements in 
4-8 (Solid Elements) 
LS-DYNA Draft
LS-DYNA Theory Manual 
Solid Elements 
this  matrix  that  needs  to  be  processed  compared  to  72  for  the  standard  solid  element 
type  2.  A  slight  modification  of  the  jacobian  matrix  will  substantially  reduce  the 
computational expense for this element.  Simply substitute the expressions for 𝜉𝑘𝑖 and 𝜉𝑙𝑖 
by  
and 
𝜉𝑘𝑖 = 𝜉𝑘𝜅𝑗𝑘,
𝜉𝑙𝑖 = 𝜉𝑙𝜅𝑗𝑙.
(4.2.39)
(4.2.40)
This will lead to a stiffness reduction for certain modes, in particular the out-of-
plane  hourglass  mode  as  can  be  seen  by  once  again  looking  at  the  transverse  shear 
locking example.  The velocity gradient for pure bending is now 
𝐿𝑖𝑖 =
4𝑙𝑖
𝐿𝑖𝑝 = 0, 
4𝑙𝑞
𝐿𝑖𝑞 =
𝜉𝑞𝜅𝑖𝑞,
𝜉𝑖𝜅𝑞𝑖, 
and if it turns out that 𝑙𝑖 is smaller than 𝑙𝑞, then this results in 
𝐿𝑖𝑖 =
4𝑙𝑞
𝜉𝑞. 
(4.2.41)
(4.2.42)
That  is,  if  𝑖  represents  the  direction  of  the  thinnest  dimension,  its  corresponding 
bending strain is inadequately reduced. 
4.2.6  Example 
A  plate  of  dimensions  10 × 5 × 1 mm3  is  clamped  at  one  end  and  subjected  to  a  1 Nm 
torque at the other end.  The Young’s modulus is 210 GPa and the analytical solution for 
the  end  tip  deflection  is  0.57143 mm.  In  order  to  study  the  mesh  convergence  for  the 
three  fully  integrated  bricks  the  plate  is  discretized  into  2 × 1 × 1,  4 × 2 × 2,  8 × 4 × 4, 
16 × 8 × 8and finally 32 × 16 × 16 elements, all elements having the same aspect ratio of 
5 × 1. The table below shows the results for the different fully integrated elements, and 
indicates an accuracy improvement for solid elements −1 and −2. 
Discretization   Solid element type 2 
2x1x1 
4x2x2 
8x4x4 
16x8x8 
32x16x16 
Solid element type -2  Solid element type -1 
0.6711 (17.4%) 
0.5466 (4.3%) 
0.5472 (4.2%) 
0.5516 (3.5%) 
0.5535 (3.1%) 
0.0564 (90.1%) 
0.1699 (70.3%) 
0.3469 (39.3%) 
0.4820 (15.7%) 
0.5340 (6.6%) 
0.6751 (18.1%) 
0.5522 (3.4%) 
0.5500 (3.8%) 
0.5527 (3.3%) 
0.5540 (3.1%) 
4.3  Hourglass Control 
The biggest disadvantage to one-point integration is the need to control the zero 
energy  modes,  which  arise,  called  hourglassing  modes.    Undesirable  hourglass  modes 
tend to have periods that are typically much shorter than the periods of the structural
Solid Elements 
LS-DYNA Theory Manual 
response, and they are often observed to be oscillatory.  However, hourglass modes that 
have  periods  that  are  comparable  to  the  structural  response  periods  may  be  a  stable 
kinematic  component  of  the  global  deformation  modes  and  must  be  admissible.    One 
way  of  resisting  undesirable  hourglassing  is  with  a  viscous  damping  or  small  elastic 
stiffness  capable  of  stopping  the  formation  of  the  anomalous  modes  but  having  a 
negligible  affect  on  the  stable  global  modes.    Two  of  the  early  three-dimensional 
algorithms for controlling the hourglass modes were developed by Kosloff and Frazier 
[1974] and Wilkins et al.  [1974]. 
Since the hourglass deformation modes are orthogonal to the strain calculations, 
work  done  by  the  hourglass  resistance  is  neglected  in  the  energy  equation.    This  may 
lead to a slight loss of energy; however, hourglass control is always recommended for 
the  under  integrated  solid  elements.    The  energy  dissipated  by  the  hourglass  forces 
reacting  against  the  formations  of  the  hourglass  modes  is  tracked  and  reported  in  the 
output files matsum and glstat. 
It  is  easy  to  understand  the  reasons  for  the  formation  of  the  hourglass  modes.  
Consider the following strain rate calculations for the 8-node solid element 
𝜀̇𝑖𝑗 =
(∑
𝑘=1
∂𝜙𝑘
∂𝑥𝑖
𝑥̇𝑗
+
∂𝜙𝑘
∂𝑥𝑗
𝑘).
𝑥̇𝑖
Whenever diagonally opposite nodes have identical velocities, i.e., 
7,
1 = 𝑥̇𝑖
𝑥̇𝑖
8,
2 = 𝑥̇𝑖
𝑥̇𝑖
5,
3 = 𝑥̇𝑖
𝑥̇𝑖
6,
4 = 𝑥̇𝑖
𝑥̇𝑖
(4.43)
(4.44)
1k
3k
2k
4k
Figure  4.3.    The  hourglass  modes  of  an  eight-node  element  with  one
integration point are shown  [Flanagan and Belytschko 1981].  A total of twelve
modes exist.
LS-DYNA Theory Manual 
Solid Elements 
𝛼 = 1 𝛼 = 2 𝛼 = 3 𝛼 = 4
1 
-1 
1 
-1 
-1 
1 
-1 
1 
1 
-1 
-1 
1 
-1 
1 
1 
-1 
1 
-1 
1 
-1 
1 
-1 
1 
-1 
1 
1 
-1 
-1 
-1 
-1 
1 
1 
𝛤𝑗1 
𝛤𝑗2 
𝛤𝑗3 
𝛤𝑗4 
𝛤𝑗5 
𝛤𝑗6 
𝛤𝑗7 
𝛤𝑗8 
Table 4.  Hourglass base vectors. 
the strain rates are identically zero: 
𝜀̇𝑖𝑗 = 0,
(4.45)
due to the asymmetries in Equations (4.15).  It is easy to prove the orthogonality of the 
hourglass  shape  vectors,  which  are  listed  in  Table  4  and  shown  in  Figure  4.3  with  the 
derivatives of the shape functions: 
∑
𝑘=1
∂𝜙𝑘
∂𝑥𝑖
𝛤𝛼𝑘 = 0
,
𝑖 = 1, 2, 3,
𝛼 = 1, 2, 3, 4.
(4.46)
The  product  of  the  base  vectors  with  the  nodal  velocities  is  zero  when  the  element 
velocity field has no hourglass component, 
ℎ𝑖𝛼 = ∑ 𝑥̇𝑖
𝑘𝛤𝛼𝑘
= 0. 
(4.47)
𝑘  
are nonzero if hourglass modes are present.  The 12 hourglass-resisting force vectors, 𝑓𝑖𝛼
are 
𝑘=1
where 
𝑘 = 𝑎ℎℎ𝑖𝛼𝛤𝛼𝑘,
𝑓𝑖𝛼
3⁄ 𝑐
𝑎ℎ = 𝑄HG𝜌𝑣e
,
(4.48)
(4.49)
in  which  𝑣e  is  the  element  volume,  𝑐  is  the  material  sound  speed,  and  𝑄HG  is  a  user-
defined constant usually set to a value between .05 and .15.  Equation (1.21) is hourglass 
control type 1 in the LS-DYNA User’s Manual. 
A  shortcoming  of  hourglass  control  type  1  is  that  the  hourglass  resisting  forces  of 
Equation (1.21) are not orthogonal to linear velocity field when elements are not in the 
shape  of  parallelpipeds.    As  a  consequence,  such  elements  can  generate  hourglass 
energy  with  a  constant  strain  field  or  rigid  body  rotation.    Flanagan  and  Belytschko 
[1981]  developed  an  hourglass  control  that  is  orthogonal  to  all  modes  except  the  zero 
energy hourglass modes.  Instead of resisting components of the bilinear velocity field 
that are orthogonal to the strain calculation, Flanagan and Belytschko resist components
Solid Elements 
LS-DYNA Theory Manual 
of the velocity field that are not part of a fully linear field.  They call this field, defined 
below, the hourglass velocity field 
𝑘HG
𝑥̇𝑖
= 𝑥̇𝑖
𝑘 − 𝑥̇𝑖
𝑘LIN
,
where 
and 
𝑘LIN
𝑥̇𝑖
= 𝑥̅
̇i + 𝑥̅
̇𝑖,𝑗(𝑥𝑗
𝑘 − 𝑥̅𝑗),
𝑥̅𝑖 =
̇𝑖 =
𝑥̅
𝑘,
∑ 𝑥𝑖
𝑘=1
∑ 𝑥̇𝑖
𝑘=1
. 
(4.50)
(4.51)
(4.52)
Flanagan  and  Belytschko  construct  geometry-dependent  hourglass  shape  vectors  that 
are  orthogonal  to  the  fully  linear  velocity  field  and  the  rigid  body  field.    With  these 
vectors  they  resist  the  hourglass  velocity  deformations.    Defining  hourglass  shape 
vectors in terms of the base vectors as 
the analogue for (4.47) is, 
𝛾𝛼𝑘 = 𝛤𝛼𝑘 − 𝜙𝑘,𝑖 ∑ 𝑥𝑖
𝛤𝛼𝑛,
𝑛=1
𝑔𝑖𝛼 = ∑ 𝑥̇𝑖
𝑘=1
𝛾𝛼𝑘 = 0,
with the 12 resisting force vectors being 
𝑘 = 𝑎ℎ𝑔𝑖𝛼𝛾𝛼𝑘,
𝑓𝑖𝛼
(4.53)
(4.54)
(4.55)
where  𝑎ℎ  is  a  constant  given  in  Equation  (4.48).    Equation  (1.28)  corresponds  to 
hourglass control type 2 in the LS-DYNA User’s Manual.  The 𝛾 terms used of equation 
of Equation (1.26) are used not only type hourglass control type 2, but are the basis for 
all solid element hourglass control except for form 1.  
A cost comparison in Table 4.1 shows that the default type 1 hourglass viscosity 
requires  approximately  130  adds  or  multiplies  per  hexahedron,  compared  to  620  and 
680  for  the  algorithms  of  Flanagan-Belytschko  and  Wilkins.    Therefore,  for  a  very 
regular  mesh,  type  1  hourglass  control  may  provide  a  faster,  sufficiently  accurate 
solution, but in general, any of the other hourglass options which are all based on the 
𝛾𝛼𝑘 terms of Equation (1.26) will be a better choice. 
Type  3  hourglass  control  is  identical  to  type  2,  except  that  the  shape  function 
derivatives in Eq.  (1.26) are evaluated at the centroid of the element rather than at the 
origin of the referential coordinate system.  With this method, Equation (1.14) produces 
the exact element volume.  However, the anti-symmetry property of Equation (1.15) is 
not true, so there is some increased number of computations.
LS-DYNA Theory Manual 
Solid Elements 
The  remaining  hourglass  control  types  calculated  hourglass  forces  proportional 
to  total  hourglass  deformation  rather  than  hourglass  viscosity.    A  stiffness  form  of 
hourglass  control  allows  elements  to  spring  back  and  will  absorb  less  energy  than  the 
viscous forms. 
Types  4  and  5  hourglass  control  are  similar  to  types  2  and  3,  except  that  they 
evaluate hourglass stiffness rather than viscosity.  The hourglass rates of equation (1.27) 
are  multiplied  by  the  solution  time  step  to  produce  increments  of  hourglass 
deformation.  The hourglass stiffness is scaled by the element’s maximum frequency so 
that  stability  can  is  maintained  as  long  as  the  hourglass  scale  factor,  𝑎ℎ,  is  sufficiently 
small. 
Type 6 hourglass control improves on type 5 by scaling the stiffness such that the 
hourglass forces match those generated by a fully integrated element control by doing 
closed  form  integration  over  the  element  volume  scaling  the  hourglass  stiffness  by 
matching  the  stabilization  for  the  3D  hexahedral  element  is  available  for  both  implicit 
and  explicit  solutions.    Based  on  material  properties  and  element  geometry,  this 
stiffness type stabilization is developed by an assumed  strain method [Belytschko and 
Bindeman  1993]  such  that  the  element  does  not  lock  with  nearly  incompressible 
material.    When  the  user  defined  hourglass  constant  𝑎h  is  set  to  1.0,  accurate  coarse 
mesh bending stiffness is obtained for elastic material.  For nonlinear material, a smaller 
value  of  𝑎h  is  suggested  and  the  default  value  is  set  to  0.1.    In  the  implicit  form,  the 
assumed strain stabilization matrix is: 
𝐊stab = 2𝜇𝑎h
𝐤11 𝐤12 𝐤13
⎤
𝐤21 𝐤22 𝐤23
, 
⎥
𝐤31 𝐤32 𝐤33⎦
⎡
⎢
⎣
where the 8 × 8 submatricies are calculated by: 
𝐤𝑖𝑖 ≡ 𝐻𝑖𝑖 [(
) (𝛄𝑗𝛄𝑗
𝐤𝑖𝑗 ≡ 𝐻𝑖𝑗 [(
, 
) 𝛄𝑗𝛄𝑖
T +
1 − 𝜐
1 − 𝜐
T + 𝛄𝑘𝛄𝑘
𝛄𝑖𝛄𝑗
T]
T) + (
1 + 𝜐
) 𝛄4𝛄4
T] +
(𝐻𝑗𝑗 + 𝐻𝑘𝑘)𝛄𝑖𝛄1
T, 
with, 
where, 
𝐻𝑖𝑖 ≡ ∫(ℎ𝑗,𝑖)
𝐻𝑖𝑗 ≡ ∫ ℎ𝑖,𝑗ℎ𝑗,𝑖
𝑑𝑣 = ∫(ℎ𝑘,𝑖)2
𝑑𝑣 = 3 ∫(ℎ4,𝑖)2
𝑑𝑣, 
𝑑𝑣, 
ℎ1 = 𝜉𝜂    ℎ2 = 𝜂𝜁
ℎ3 = 𝜁𝜉
ℎ4 = 𝜉𝜂𝜁 ,
(4.56)
(4.57)
(4.58)
(4.59)
Subscripts  𝑖,  𝑗,  and  𝑘  are  permuted  as  in  Table  44.2.    A  comma  indicates  a 
derivative  with  respect  to  the  spatial  variable  that  follows.    The  hourglass  vectors,  𝛾𝛼 
are  defined  by  equation  (4.53).    The  stiffness  matrix  is  evaluated  in  a  corotational
Solid Elements 
LS-DYNA Theory Manual 
1 
1 
2 
2 
3 
3 
2 
3 
3 
1 
1 
2 
3 
2 
1 
3 
2 
1 
Table 44.2.  Permutations of i, j, and k. 
coordinate system that is aligned with the referential axis of the element.  The use of a 
corotational  system  allows  direct  evaluation  of  integrals  in  equations  (4.58)  by 
simplified equations that produce a more accurate element than full integration. 
T𝐱𝑗)(𝚲𝑘
T𝐱𝑖)
(𝚲𝑖
𝑖 ≠ 𝑗 ≠ 𝑘,
𝐻𝑖𝑖 =
T𝐱𝑘)
(𝚲𝑗
(4.60)
𝐻𝑖𝑗 =
(𝚲𝑘
T𝐱𝑘)
𝑖 ≠ 𝑗 ≠ 𝑘,
(4.61)
Λ𝑖 are 8 × 1 matrices of the referential coordinates of the nodes as given in Figure 4.1, 
and x𝑖 are 8 × 1 matrices of the nodal coordinates in the corotational system.  For each 
material type, a Poisson's ratio, 𝑣, and an effective shear modulus, 𝜇, is needed. 
In the explicit form, the 12 hourglass force stabilization vectors are 
stab = ∑ 𝑎h𝑔𝑖𝛼𝛄𝛼
𝐟𝑖
𝛼=1
,
where the 12 generalized stresses are calculated incrementally by 
𝑛 = 𝑔𝑖𝛼
𝑔𝑖𝛼
𝑛−1 + Δ𝑡𝑔̇𝑖𝛼
𝑛−1
2,
𝑔̇𝑖𝑖 = 𝜇[(𝐻𝑗𝑗 + 𝐻𝑘𝑘)𝑞 ̇𝑖𝑖 + 𝐻𝑖𝑗𝑞 ̇𝑗𝑗 + 𝐻𝑖𝑘𝑞 ̇𝑘𝑘],
, 
𝑔̇𝑖𝑗 = 2𝜇 [
, 
𝑔̇𝑖4 = 2𝜇 (
1 − 𝜐
1 + 𝜈
𝐻𝑖𝑖𝑞 ̇𝑖𝑗 + 𝜐𝐻𝑘𝑘𝑞 ̇𝑖𝑖]
) 𝐻𝑖𝑖𝑞 ̇𝑖4
and 
where, 
(4.62)
(4.63)
(4.64)
T𝐱̇𝑖).
Subscripts  𝑖, 𝑗, and 𝑘  are  permuted  as  per  Table  44.2.    As  with  the  implicit  form, 
calculations are done in a corotational coordinate system in order to use the simplified 
equations (4.60) and (4.61). 
𝑞 ̇𝑖𝛼 = (𝛄𝛼
(4.65)
LS-DYNA Theory Manual 
Solid Elements 
Type  7  hourglass  control  is  very  similar  to  type  6  hourglass  control  but  with  one 
significant difference.  As seen in Equation (1.36), type 6 obtains the current value of the 
generalized stress from the previous value and the current increment.  The incremental 
method is nearly always sufficiently accurate, but it is possible for hourglass modes to 
fail to spring back to the initial element geometry since the hourglass stiffness varies as 
the  H  terms  given  by  Equations  (1.33)  and  (1.34)  are  recalculated  in  the  deformed 
configuration  each  cycle.    Type  7  hourglass  control  eliminates  this  possible  error  by 
calculating the total hourglass deformation in each cycle.  For type 7 hourglass control, 
Equations (1.37) are rewritten using 𝑔 and 𝑞 in place of 𝑔̇ and 𝑞 ̇, and Equation (1.38) is 
replaced by (1.39). 
𝑞𝑖𝛼 = (𝛄𝛼
T𝐱𝑖) − (𝛄0𝛼
In  Equation  (1.39),  𝐱𝟎𝒊  and  𝛄𝟎𝜶  are  evaluated  using  the  initial,  undeformed  nodal 
coordinate values.  Type 7 hourglass control is considerably slower than type 6, so it is 
not  generally  recommended,  but  may  be  useful  when  the  solution  involves  at  least 
several  cycles  of  loading  and  unloading  that  involve  large  element  deformation  of 
elastic or hyperelastic material. 
T 𝐱0𝑖).
(4.39)
Both type 6 and 7 hourglass control are stiffness type methods, but may have viscosity 
added  through  the  VDC  parameter  on  the  *HOURGLASS  card.    The  VDC  parameter 
scales  the  added  viscosity,  and  VDC = 1.0  corresponds  approximately  to  critical 
damping.  The primary motivation for damping is to reduce high frequency oscillations.  
A  small  percentage  of  critical  damping  should  be  sufficient  for  this,  but  it  is  also 
possible  to  add  supercritical  damping  along  with  a  small  value  of  QM  to  simulate  a 
very viscous material that springs back slowly.
4.4  Puso Hourglass Control 
Regarding  the  solid  elements  in  LS-DYNA,  the  fully  integrated  brick  uses 
selective-reduced  integration,  which  is  known  to  alleviate  volumetric  locking  but  not 
shear  locking  for  elements  with  poor  aspect  ratio.    The  enhanced  assumed  strain 
methods have been the most successful at providing coarse mesh accuracy for general 
non-linear  material  models.    In  short,  these  elements  tend  to  sacrifice  computational 
efficiency  for  accuracy  and  are  hence  of  little  interest  in  explicit  analysis.    Puso  [2000] 
developed  an  enhanced  assumed  strain  element  that  combines  coarse  mesh  accuracy 
with  computational  efficiency.    It  is  formulated  as  a  single  point  integrated  brick  with 
  In  this  project,  we  have 
an  enhanced  assumed  strain  physical  stabilization. 
implemented this element in LS-DYNA and made comparisons with the assumed strain 
element  developed  by  Belytschko  and  Bindeman  [1993]  to  see  whether  it  brings 
anything new to the existing LS-DYNA element library.  This is hourglass control type 
9.
Solid Elements 
LS-DYNA Theory Manual 
The element formulation is that of Puso [2000], and is essentially the mean strain 
hexahedral  element  by  Flanagan  and  Belytschko  [1981]  in  which  the  perturbation 
hourglass control is substituted for an enhanced assumed strain stabilization force. 
Given the matrices 
𝐒 =
⎤
⎡
⎥
⎢
⎥
⎢
⎥
⎢
⎥
⎢
⎥
⎢
⎥
⎢
⎥
⎢
⎥
⎢
1⎦
⎣
,
𝚵 =
−1 −1 −1
⎤
1 −1 −1
⎥
1 −1
⎥
⎥
1 −1
−1
⎥
⎥
−1 −1
⎥
1 −1
⎥
⎥
1⎦
−1
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
,
𝐇 =
we can define the vector of shape functions as 
1 −1 −1
1 −1
⎤
⎥
−1 −1
1 −1
⎥
⎥
−1
1 −1
⎥
, 
⎥
−1 −1
⎥
−1
1 −1 −1
⎥
⎥
1 −1 −1 −1⎦
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
where 
The position vector 
𝐍(𝛏) =
[𝐬 + 𝚵𝛏 + 𝐇𝐡(𝛏)],
𝛏 =
⎤ ,
⎡
⎥
⎢
𝜍⎦
⎣
𝐡(𝛏) =
𝜂𝜍
⎤
𝜉𝜍
⎥⎥⎥
. 
𝜉𝜂
𝜉𝜂𝜍⎦
⎡
⎢⎢⎢
⎣
𝐱(𝛏) =
𝑥(𝛏)
⎤
𝑦(𝛏)
, 
⎥
𝑧(𝛏)⎦
⎡
⎢
⎣
is for isoparametric finite elements given as 
𝐱(𝛏) = 𝐗T𝐍(𝛏),
where 
(4.66)
(4.67)
(4.68)
(4.69)
(4.70)
𝑦1
𝑦2
𝑦3
𝑦4
𝑦5
𝑦6
𝑦7
𝑦8
is the matrix of nodal coordinates.  The Jacobian matrix maps the isoparametric domain 
to the physical domain as 
𝑧1
⎤
𝑧2
⎥
𝑧3
⎥
⎥
𝑧4
⎥
, 
𝑧5
⎥
⎥
𝑧6
⎥
⎥
𝑧7
𝑧8⎦
𝑥1
⎡
𝑥2
⎢
𝑥3
⎢
⎢
𝑥4
⎢
𝑥5
⎢
⎢
𝑥6
⎢
⎢
𝑥7
𝑥8
⎣
𝐗 =
(4.71)
and we find the Jabobian matrix at the element centroid to be 
𝐉(𝛏) =
∂𝐱(𝛏)
∂𝛏
,
(4.72)
LS-DYNA Theory Manual 
Solid Elements 
We  may  use  this  to  rewrite  the  vector  of  shape  functions  partially  in  terms  of  the 
position vector as 
𝐉0 = 𝐉(0) =
𝐗T𝚵.
(4.73)
Where 
𝐍(𝛏) = 𝐛0 + 𝐁0𝐱 + 𝚪𝐡(𝛏),
𝐛0 =
𝚪 =
𝐁0 =
{𝐈 − 𝐁0𝐗T}𝐬 ,
{𝐈 − 𝐁0𝐗T}𝐇,
−1
𝚵𝐉0
.
The gradient-displacement matrix from this expression is given as 
where 
We have 
𝐁(𝛏) = 𝐁0 + 𝐁𝑠(𝛏),
𝐁𝑠(𝛏) = 𝚪
∂𝐡(𝛏)
∂𝛏
𝐉(𝛏)−1.
∂𝐡(𝛏)
∂𝛏
=
𝜂𝜍
⎡
⎢
⎢
⎢
⎣
𝜉𝜍
⎤
⎥
. 
⎥
⎥
𝜉𝜂⎦
(4.74)
(4.75a)
(4.75b)
(4.75c)
(4.76)
(4.77)
(4.78)
At  this  point  we  substitute  the  gradient-displacement  matrix  at  the  centroid  of  the 
element 𝐁0 with the mean gradient-displacement matrix 𝐁 defined as 
𝐁 =
𝑉𝑒
∫ 𝐁(𝛏)𝑑𝑉𝑒
,
(4.79)
where 𝑒 refers to the element domain and 𝑉𝑒 is the volume of the element, in all of the 
expressions above.  That is 
and 
where 
𝚪 =
{𝐈 − 𝐁𝐗T}𝐇,
𝐁(𝛏) = 𝐁 + 𝐁𝑠(𝛏),
𝐁𝑠(𝛏) = 𝚪
∂𝐡(𝛏)
∂𝛏
𝐉(𝛏).
Proceeding, we write the expression for the rate-of-deformation as 
(4.80)
(4.81)
(4.82)
Solid Elements 
LS-DYNA Theory Manual 
𝛆̇ =
=
=
=
[𝐗̇ T𝐁(𝛏) + 𝐁(𝛏)T𝐗̇] 
(𝐗̇ T
𝐁 + 𝐁
(𝐗̇ T
𝐁 + 𝐁
𝐗̇ ) +
𝐗̇ ) +
(𝐗̇ T
𝐁 + 𝐁
𝐗̇) +
𝐗̇ T𝚪
[𝐗̇ T𝐁𝑠(𝛏) + 𝐁𝑠(𝛏)T𝐗̇ ] 
{⎧
2 ⎩{⎨
𝐉(𝛏)−T
∂𝐡(𝛏)
∂𝛏
{⎧
⎩{⎨
𝐉(𝛏)T𝐗̇ T𝚪
∂𝐡(𝛏)
∂𝛏
𝐉(𝛏)−1 + 𝐉(𝛏)−T [
∂𝐡(𝛏)
∂𝛏
∂𝐡(𝛏)
∂𝛏
]
]
𝐗̇
}⎫
⎭}⎬
}⎫
𝐗̇𝐉(𝛏)
⎭}⎬
+ [
(4.83)
𝐉(𝛏)−1,
where  we  substitute  the  occurrences  of  the  jacobian  matrix  𝐉(ξ)with  the  following 
expressions 
𝛆̇ ≈
(𝐗̇ T
𝐁 + 𝐁
𝐗̇) +
−T
𝐉̂0
{⎧
⎩{⎨
T𝐗̇ T𝚪
𝐉0
∂𝐡(𝛏)
∂𝛏
+ [
∂𝐡(𝛏)
]
∂𝛏
𝚪T𝐗̇𝐉0
}⎫
⎭}⎬
−1, 
𝐉̂0
where 
𝐉̂0 =
∥𝐣1∥
⎡
⎢
⎣
∥𝐣2∥
⎤
, 
⎥
∥𝐣3∥⎦
(4.84)
(4.85)
and j𝑖 is the i:th column in the matrix 𝐉0. This last approximation is the key to the mesh 
distortion insensitivity that characterizes the element. 
Changing to Voigt notation, we define the stabilization portion of the strain rate 
as 
where now 
−1 =
𝐉0
∥𝐣1∥−2
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
𝛆̇𝑠 = 𝐉̂0
−1𝐁̃𝑠(𝛏)𝐮̇
̃,
∥𝐣2∥−2
∥𝐣3∥−2
∥𝐣1∥−1∥𝐣2∥−1
∥𝐣3∥−1∥𝐣2∥−1
⎤
⎥
⎥
⎥
⎥
, 
⎥
⎥
⎥
⎥
⎥
∥𝐣1∥−1∥𝐣3∥−1⎦
𝐁̃𝑠(𝛏) =
γ2𝜍 + γ3𝜂 + γ4𝜍𝜂
⎡
⎢
⎢
⎢
⎢
γ1𝜍
⎢
⎢
⎢
γ1𝜂
⎣
γ1𝜍 + γ3𝜉 + γ4𝜍𝜉
γ2𝜍
γ2𝜉
γ1𝜂 + γ2𝜉 + γ4𝜉𝜂
γ3𝜉
γ3𝜂
⎤
⎥
⎥
⎥
, 
⎥
⎥
⎥
⎥
⎦
(4.86)
(4.87)
(4.88)
̃  is  the  vector  of  nodal  velocities  transformed  to  the  isoparametric  system 
and  𝐮̇
according to
LS-DYNA Theory Manual 
Solid Elements 
where  𝕵  is  the  24 × 24  matrix  that  transforms  the  8  nodal  velocity  vectors  to  the 
isoparametric domain given by 
𝐮̇
̃ = 𝕵𝐮̇,
(4.89)
𝕵 = perm
𝐉0
⎡
⎢⎢
⎣
⋱
⎤
. 
⎥⎥
T⎦
𝐉0
(4.90)
Moreover,  𝛄𝑖  is  the  ith  row  of  𝚪
parallelepiped finite elements to lock in shear. 
.    We  have  deliberately  neglected  terms  that  cause 
To  eliminate  Poisson  type  locking  in  bending  and  volumetric  locking,  an 
enhanced isoparametric rate-of-strain field is introduced as 
with 
𝛆̇𝑒 = 𝐉̂0
−1𝐆̃(𝛏)𝛂̇,
𝜂 0
Hence, the stabilized strain field becomes 
𝐆̃(𝛏) =
⎡
⎢
⎢
⎢
⎢
⎢
⎣
𝜉𝜂 𝜂𝜍
𝜉𝜂 𝜂𝜍
𝜉𝜂 𝜂𝜍
𝜍𝜉
⎤
𝜍𝜉
⎥
⎥
𝜍𝜉
. 
⎥
⎥
⎥
0 ⎦
𝛆̇𝑠 = 𝐉̂0
−1[𝐁̃𝑠(𝛏)𝐮̇
̃ + 𝐆̃(𝛏)𝛂̇] = 𝐉̂0
−1𝛆̇
̃𝑠,
(4.91)
(4.92)
(4.93)
where  𝜶̇  is  the  enhanced  strain  vector  that  must  be  determined  from  an  equilibrium 
condition.  
The virtual work equation can be written 
𝛿𝑊int = ∫ 𝛿𝛆T𝛔𝐝𝑉𝑒
, 
= ∫ 𝛿𝛆T𝐽−1𝐉T𝐒𝑑𝑉𝑒
, 
= ∫ 𝛿𝛆T𝐽−1𝐉T
= ∫ 𝛿𝛆T𝐽−1𝐉T
⎜⎛∫ 𝐂𝑆𝐸𝐄̇𝑑𝜏
⎝
⎟⎞ 𝑑𝑉𝑒
⎠
, 
⎜⎛∫ 𝐽𝐉−T𝐂𝜎𝛆̇𝑑𝜏
⎝
⎟⎞ 𝑑𝑉𝑒
⎠
, 
= ∫ 𝛿𝛆T𝑗0𝐉0
≈ ∫ 𝛿𝛆̃T
⎜⎛∫
⎝
⎜⎛∫ 𝐽𝐉0
⎝
𝑉𝑒
−T𝐂𝜎𝛆̇𝑑𝜏
⎟⎞ 𝑑𝑉𝑝
⎠
, 
−T𝐂𝜎𝐉̂0
𝐉̂0
−1𝛆̇
̃𝑑𝜏
⎟⎞ 𝑑𝑉𝑝
⎠
, 
(4.94a)
(4.94b)
(4.94c)
(4.94d)
(4.94e)
(4.94f)
Solid Elements 
LS-DYNA Theory Manual 
where 𝐽 is the determinant of the deformation gradient, 𝐉 is the push-forward operator 
of  a  symmetric  2nd  order  tensor,  𝑗0  is  the  determinant  of  the  jacobian  matrix,  𝑗0  is  the 
determinant of the jacobian matrix at time 0, σ is the true stress tensor, 𝐒 is the 2nd Piola-
Kirchhoff  stress  tensor,  𝐂𝑆𝐸  is  the  material  tangent  modulus,  𝐂σ  is  the  spatial  tangent 
modulus  and  𝑉𝑒  is  the  volume  of  the  element.    In  the  above,  we  have  used  various 
transformation formulae between different stress and constitutive tensors.  At this point 
we are only interested in how to handle the stabilization portion of the strain rate field, 
the  constant  part  is  only  used  to  update  the  midpoint  stress  as  usual.    Because  of 
orthogonality  properties  of  the  involved  matrices,  it  turns  out  that  we  may  just  insert 
the expression for the stabilization strain rate field to get 
𝛿𝑊int
𝑠 ≈ ∫ 𝛿𝛆̃𝑠
⎜⎛∫
⎝
𝑉𝑒
−T𝐂𝜎𝐉̂0
𝐉̂0
−1𝛆̇
̃𝑠𝑑𝜏
⎟⎞ 𝑑𝑉𝑝
⎠
,
(4.95a)
= [𝛿𝐮̃𝑇
𝛿𝜶T] ∫ [
𝚩̃𝑠(𝛏)𝑇
𝐆̃(𝛏)𝑇 ]
⎜⎛∫
⎝
𝑉𝑒
−T𝐂𝜎𝐉̂0
𝐉̂0
−1[𝚩̃𝑠(𝛏) 𝐆̃(𝛏)] [𝐮̇
𝛂̇
] 𝑑𝜏
⎟⎞ 𝑑𝑉𝑝
⎠
. 
(4.95b)
The stabilization contribution to the internal force vector is given by 
[
𝐟𝑢
𝐟𝛼
] = [𝕵T
] ∫ [
𝚩̃𝑠(𝛏)T
𝐆̃(𝛏)T ]
⎜⎛∫
⎝
𝑉𝑒
−T𝐂𝜎𝐉̂0
𝐉̂0
−1[𝚩̃𝑠(𝛏) 𝐆̃(𝛏)][𝕵 0
][𝐮̇
𝛂̇
]𝑑𝜏
⎟⎞ 𝑑𝑉𝑝
⎠
.
(4.96)
In  a  discretization,  the  condition  𝐟𝛼 = 0  is  used  to  determine  Δ𝛂,  the  increment  of  the 
enhanced  strain  variables,  from  Δu,  the  increment  in  displacements.    This  is  inserted 
back into the expression for the internal force vectors to determine 𝐟𝑢, the stabilization 
contribution to the internal force vector. 
The implementation of the element is very similar to the implementation of the 
one  point  integrated  mean  strain  hexahedral  by  Flanagan  and  Belytschko  [1981].    The 
hourglass forces are calculated in a different manner. 
From the midpoint stress update we get a bulk and shear modulus characterizing 
the  material  at  this  specific  point  in  time.    From  this  we  form  the  isotropic  spatial 
tangent  modulus  𝐂𝛔  to  be  used  for  computing  the  stabilization  force  from  Equation 
(4.96).
4.5  Fully Integrated Brick Elements and Mid-Step Strain 
Evaluation 
To  avoid  locking  in  the  fully  integrated  brick  elements  strain  increments  at  a 
point  in  a  constant  pressure,  solid  element  are  defined  by  [see  Nagtegaal,  Parks, 
anmmmmmd Rice 1974] 
4-20 (Solid Elements)
LS-DYNA Theory Manual 
Solid Elements 
Δ𝜀𝑥𝑥 =
Δ𝜀𝑦𝑦 =
∂Δ𝑢
∂𝑥𝑛+1
2⁄
∂Δ𝑣
∂𝑦𝑛+1
2⁄
Δ𝜀𝑧𝑧 =
∂Δ𝑤
∂𝑧𝑛+1
2⁄
+ 𝜙,
Δ𝜀𝑥𝑦 =
+ 𝜙,
Δ𝜀𝑦𝑧 =
+ 𝜙,
Δ𝜀𝑧𝑥 =
, 
, 
∂Δ𝑣
∂𝑥𝑛+1
2⁄
+ ∂Δ𝑢
∂𝑦𝑛+1
2⁄
∂Δ𝑤
∂𝑦𝑛+1
2⁄
∂Δ𝑢
∂𝑧𝑛+1
2⁄
+ ∂Δ𝑣
∂𝑧𝑛+1
2⁄
+ ∂Δ𝑤
∂𝑥𝑛+1
2⁄
,
(4.97)
where 𝜙 modifies the normal strains to ensure that the total volumetric strain increment 
at each integration point is identical 
𝑛+1
2⁄
𝜙 =   Δ𝜀𝑣
∂Δ𝑢
∂𝑥𝑛+1
2⁄
+ ∂Δ𝑣
∂𝑦𝑛+1
2⁄
−
+ ∂Δ𝑤
∂𝑧𝑛+1
2⁄
,
𝑛+1
2⁄
and Δ𝜀𝑣
is the average volumetric strain increment in the midpoint geometry 
∫
𝑣𝑛+1
2⁄
⎜⎜⎛ ∂Δ𝑢
∂𝑥𝑛+1
2⁄
⎝
+ ∂Δ𝑤
∂𝑧𝑛+1
2⁄
⎟⎟⎞ 𝑑𝑣𝑛+1
2⁄
⎠
, 
+ ∂Δ𝑣
∂𝑦𝑛+1
2⁄
𝑑𝑣𝑛+1
2⁄
∫
𝑣𝑛+1
2⁄
(4.98)
(4.99)
Δ𝑢,. Δ𝑣, and Δ𝑤 are displacement increments in the x, y, and z directions, respectively, 
and 
𝑥𝑛+1
2⁄ =
(𝑥𝑛 + 𝑥𝑛+1)
,
𝑦𝑛+1
2⁄ =
(𝑦𝑛 + 𝑦𝑛+1)
, 
(4.100a)
(4.100b)
2⁄ =
𝑧𝑛+1
(𝑧𝑛 + 𝑧𝑛+1)
. 
To satisfy the condition that rigid body rotations cause zero straining, it is necessary to 
use  the  geometry  at  the  mid-step  in  the  evaluation  of  the  strain  increments.    As  the 
default,  LS-DYNA  currently  uses  the  geometry  at  step  𝑛 + 1  to  save  operations; 
however, 
is  always 
recommended, and, for explicit calculations, which involve rotating parts, the mid-step 
geometry should be used especially if the number of revolutions is large.  The mid-step 
geometry can be activated either globally or for a subset of parts in the model by using 
the options on the control card, *CONTROL_ACCURACY. 
the  mid-step  strain  calculation 
implicit  calculations 
(4.100c)
for
Solid Elements 
LS-DYNA Theory Manual 
Figure 4.4.  Four node tetrahedron. 
Since  the  bulk  modulus  is  constant  in  the  plastic  and  viscoelastic  material 
models, constant pressure solid elements result.  In the thermoelastoplastic material, a 
constant  temperature  is  assumed  over  the  element.    In  the  soil  and  crushable  foam 
material, an average relative volume is computed for the element at time step 𝑛 + 1, and 
the  pressure  and  bulk  modulus  associated  with  this  relative  volume  is  used  at  each 
integration  point.   For  equations  of  state, one  pressure  evaluation is  done  per  element 
and is added to the deviatoric stress tensor at each integration point. 
The 
foregoing  procedure  requires 
the  strain-displacement  matrix 
corresponding  to  Equations  (4.66)  and  consistent  with  a  constant  volumetric  strain,  𝐁̅̅̅̅̅, 
be used in the nodal force calculations [Hughes 1980].  It is easy to show that: 
that 
𝐅 = ∫ (𝐁̅̅̅̅̅𝑛+1)
𝑣𝑛+1
𝛔𝑛+1𝑑𝑣 = ∫ (𝐁𝑛+1)
𝑣𝑛+1
𝛔𝑛+1𝑑𝑣,
(4.101)
and avoid the needless complexities of computing 𝐁̅̅̅̅̅.
4.6  Four Node Tetrahedron Element 
The four node tetrahedron element with one point integration, shown in Figure 
4.4,  is  a  simple,  fast,  solid  element  that  has  proven  to  be  very  useful  in  modeling  low 
density  foams  that  have  high  compressibility.    For  most  applications,  however,  this 
element  is  too  stiff  to  give  reliable  results  and  is  primarily  used  for  transitions  in 
meshes.  The formulation follows the formulation for the one point solid element with 
the  difference  that  there  are  no  kinematic  modes,  so  hourglass  control  is  not  needed.  
The basis functions are given by: 
𝑁1(𝑟, 𝑠, 𝑡) = 𝑟, 
𝑁2(𝑟, 𝑠, 𝑡) = 𝑠, 
4-22 (Solid Elements) 
(4.102a)
LS-DYNA Theory Manual 
Solid Elements 
𝑁3(𝑟, 𝑠, 𝑡) = 1 − 𝑟 − 𝑠 − 𝑡, 
𝑁4(𝑟, 𝑠, 𝑡) = 𝑡. 
(4.102c)
(4.102d)
If  a  tetrahedron  element  is  needed,  this  element  should  be  used  instead  of  the 
collapsed  solid  element  since  it  is,  in  general,  considerably  more  stable  in  addition  to 
being much faster.  Automatic sorting can be used, see *CONTROL_SOLID keyword, to 
segregate these elements in a mesh of 8 node solids for treatment as tetrahedrons.  
4.7  Nodal Pressure Tetrahedron 
For applications requiring a tetrahedron mesh, the volume averaged tetrahedron 
type 13 is an interesting alternative to the standard single point tetrahedron, also known 
as the 1 point nodal pressure tetrahedron.  The idea is to average the volumetric strain 
over adjacent elements to smooth the pressure response.  To this end, we assume that 𝐸 
is  the  set  of  all  such  elements  in  a  model,  and  likewise  𝑁  is  the  set  of  all  nodes 
belonging to these elements.  We introduce the indicator 
1/4 if node 𝑛 is connecting to element 𝑒
The volume of a node 𝑛 is defined as 
otherwise
𝑛 = {
𝜒𝑒
(4.103)
𝑛𝑉𝑒
(4.104)
where 𝑉𝑒 is the exact volume of element 𝑒. This allows us to define an average jacobian 
𝐽 ̅𝑒 for element 𝑒 as 
 𝑉𝑛 = ∑ 𝜒𝑒
𝑒∈𝐸
𝐽 ̅𝑒 = ∑ 𝜒𝑒
𝑛 {
𝑛∈𝑁
𝑉𝑛
0}
𝑉𝑛
(4.105)
0 is the nodal volume in the reference 
which is essentially the relative volume.  Here 𝑉𝑛
configuration.  The element is completely defined by the assumed deformation gradient 
given as 
𝑭̅𝑒 = (
1/3
𝐽 ̅𝑒
𝐽𝑒
)
𝑭𝑒 
(4.106)
where 𝑭𝑒  is  the  deformation  gradient  from  the  isoparametric  shape  functions  and  𝐽𝑒 =
det𝑭𝑒, also given as 
𝐽𝑒 =
𝑉𝑒
0. 
𝑉𝑒
(4.107)
The assumed rate of deformation, derived from 𝑭̅𝑒, is given as 
𝛿𝐽𝑒
𝐽𝑒
meaning that the volumetric strain is replaced by that of the averaged one.  Continuing, 
the virtual work equation is given as 
) 𝑰 + 𝛿𝑭𝑒𝑭𝑒
𝛿𝜺̅𝑒 =
−1 
(4.108)
−
(
𝛿𝐽 ̅𝑒
𝐽 ̅𝑒
LS-DYNA Draft 
∑ 𝒇𝑛
𝑛∈𝑁
𝑇𝛿𝒙𝑛
= ∑ 𝝈𝑒: 𝛿𝜺̅𝑒𝐽𝑒𝑉𝑒
𝑒∈𝐸
Solid Elements 
LS-DYNA Theory Manual 
Figure 4.5.  Six node Pentahedron. 
which  provides  the  equation  for  the  nodal  forces,  𝒇𝑛.  An  expression  for  the  strain-
𝑛,  is  deduced  from  combining  (4.108)  and  the  relation  𝛿𝜺̅𝑒 =
displacement  matrix,  𝑩𝑒
∑ 𝑩𝑒
𝑛∈𝑁
. It turns out to be given as 
𝑛𝛿𝒙𝑛
𝑛 and 𝑩̃𝑒
𝑛 = ∑ ∑ 𝜒𝑓
𝑩𝑒
𝑓 ∈𝐸
𝑚 𝑉𝑓 𝜒𝑒
𝐽 ̅𝑒𝑉𝑚
𝑛 are the volumetric and deviatoric parts of the standard (derived from 
where 𝑩̅̅̅̅̅𝑒
isoparametric  shape  functions)  strain  displacement  matrix.    Noticable  is  that  the 
support for the assumed strain displacement is not restricted to the nodal connectivity 
of a single element but is spread over a region of adjacent elements.  This renders a less 
sparse stiffness matrix, but also explains the smoothening effect of the pressure.
𝑛 
+ 𝑩̃𝑒
𝑩̅̅̅̅̅𝑓
𝑚∈𝑁
(4.110)
4.8  Six Node Pentahedron Element 
The  pentahedron  element  with  two  point  Gauss  integration  along  its  length, 
shown  in  Figure  4.5,  is  a  solid  element  that  has  proven  to  be  very  useful  in  modeling 
axisymmetric  structures  where  wedge  shaped  elements  are  used  along  the  axis-of-
revolution.    The  formulation  follows  the  formulation  for  the  one  point  solid  element 
with the difference that, like the tetrahedron element, there are no kinematic modes, so 
hourglass control is not needed.  The basis functions are given by: 
𝑁1(𝑟, 𝑠, 𝑡) =
𝑁2(𝑟, 𝑠, 𝑡) =
(1 − 𝑡)𝑟, 
(1 − 𝑡)(1 − 𝑟 − 𝑠), 
(4.111a)
(4.111b)
LS-DYNA Theory Manual 
Solid Elements 
15
16
17
20
13
11
12
19
14
18
10
DOF
ui, vi, wi
DOF 
ui, vi, wi, θ
xi, θ
yi, θ
zi
Figure 4.6.  The 20-node solid element is transformed to an 8-node solid with 6 
degrees-of-freedom per node. 
𝑁3(𝑟, 𝑠, 𝑡) =
𝑁4(𝑟, 𝑠, 𝑡) =
𝑁5(𝑟, 𝑠, 𝑡) =
𝑁6(𝑟, 𝑠, 𝑡) =
(1 + 𝑡)(1 − 𝑟 − 𝑠), 
(1 + 𝑡)𝑟, 
(1 − 𝑡)𝑠, 
(1 + 𝑡)𝑠. 
(4.111c)
(4.111d)
(4.111e)
(4.111f)
If  a  pentahedron  element  is  needed,  this  element  should  be  used  instead  of  the 
collapsed  solid  element  since  it  is,  in  general,  more  stable  and  significantly  faster.  
Automatic  sorting  can  be  used,  see  *CONTROL_SOLID  keyword,  to  segregate  these 
elements in a mesh of 8 node solids for treatment as pentahedrons.   Selective-reduced 
integration  is  used  to  prevent  volumetric  locking,  i.e.,  a  constant  pressure  over  the 
domain of the element is assumed.
4.9  Fully Integrated Brick Element With 48 Degrees-of-
Freedom 
The forty-eight degree of freedom brick element is derived from the twenty node 
solid element; see Figure 4.6, through a transformation of the nodal displacements and 
rotations of the mid-side nodes [Yunus, Pawlak, and Cook, 1989].  This element has the
Solid Elements 
LS-DYNA Theory Manual 
Figure 4.7.  A typical element edge is shown from [Yunus, Pawlak, and Cook,
1989]. 
advantage that shell nodes can be shared with brick nodes and that the faces have just 
four  nodes  —  a  real  advantage  for  the  contact-impact  logic.    The  accuracy  of  this 
element  is  relatively  good  for  problems  in  linear  elasticity  but  degrades  as  Poisson’s 
ratio approaches the incompressible limit.  This can be remedied by using incompatible 
modes in the element formulation, but such an approach seems impractical for explicit 
computations. 
The  instantaneous  velocity  for  a  midside  node  𝑘  is  given  as  a  function  of  the 
corner node velocities as , 
(𝑢̇𝑖 + 𝑢̇𝑗) +
(𝑣̇𝑖 + 𝑣̇𝑗) +
𝑢̇𝑘 =
𝑣̇𝑘 =
𝑤̇ 𝑘 =
𝑦𝑗 − 𝑦𝑖
𝑧𝑗 − 𝑧𝑖
𝑥𝑗 − 𝑥𝑖
𝑧𝑗 − 𝑧𝑖
𝑥𝑗 − 𝑥𝑖
𝑦𝑗 − 𝑦𝑖
(𝑤̇ 𝑖 + 𝑤̇ 𝑗) +
(𝜃̇
𝑦𝑗 − 𝜃̇
𝑦𝑖) +
(𝜃̇
𝑥𝑖 − 𝜃̇
𝑥𝑗), 
(𝜃̇
𝑧𝑗 − 𝜃̇
𝑧𝑖) +
(𝜃̇
𝑦𝑖 − 𝜃̇
𝑦𝑗), 
(𝜃̇
𝑥𝑗 − 𝜃̇
𝑥𝑖) +
(𝜃̇
𝑧𝑖 − 𝜃̇
𝑧𝑗), 
(4.112)
where  𝑢,  𝑣,  𝑤,  𝜃𝑥,  𝜃𝑦,  and  𝜃z  are  the  translational  and  rotational  displacements  in  the 
global 𝑥, 𝑦, and 𝑧 directions.  The velocity field for the twenty-node hexahedron element 
in terms of the nodal velocities is: 
{⎧𝑢̇
}⎫
𝑣̇
𝑤̇ ⎭}⎬
⎩{⎨
=
𝜙1 𝜙2 … 𝜙20
⎡
0 … 0
⎢
0 … 0
⎣
0 … 0
𝜙1 𝜙2 … 𝜙20
0 … 0
0 … 0
⎤
0 … 0
⎥
𝜙1 𝜙2 … 𝜙20⎦
⎧ 𝑢̇1
⎫
}}}
{{{
⋮
𝑢̇20
}}}
{{{
𝑣̇1
}
{
⋮
⎬
⎨
}}}}
{{{{
𝑣̇20
𝑤̇ 1
}}}
{{{
⋮
𝑤̇ 20⎭
⎩
, 
(4.113)
where 𝜙𝑖 are given by [Bathe and Wilson 1976] as,
LS-DYNA Theory Manual 
Solid Elements 
DOF
ui, vi, wi
DOF
ui, vi, wi, θ
xi, θ
yi, θ
zi
Figure  4.8.    Twenty-four  degrees  of  freedom  tetrahedron  element  [Yunus, 
Pawlak, and Cook, 1989]. 
𝜙1 = 𝑔1 −
𝜙2 = 𝑔2 −
𝜙3 = 𝑔3 −
,
(𝑔9 + 𝑔12 + 𝑔17)
(𝑔9 + 𝑔10 + 𝑔18)
,
(𝑔10 + 𝑔11 + 𝑔19)
(𝑔11 + 𝑔12 + 𝑔20)
𝜙5 = 𝑔5 −
𝜙6 = 𝑔6 −
,
𝜙7 = 𝑔7 −
𝜙8 = 𝑔8 −
, 
(𝑔13 + 𝑔16 + 𝑔17)
(𝑔13 + 𝑔14 + 𝑔18)
, 
(𝑔14 + 𝑔15 + 𝑔19)
(𝑔15 + 𝑔16 + 𝑔20)
, 
, 
𝜙4 = 𝑔4 −
𝜙𝑖 = 𝑔𝑖 for 𝑗 = 9, … , 20 
𝑔𝑖 = 𝐺(𝜉 , 𝜉𝑖)𝐺(𝜂, 𝜂𝑖)𝐺(𝜁 , 𝜁𝑖), 
,
𝐺(𝛽, 𝛽𝑖) =
{⎧1
⎩{⎨
(1 + 𝛽𝛽𝑖)
1 − 𝛽2
for,   𝛽𝑖 = ±1;     𝛽 = 𝜉 , 𝜂, 𝜁
 .  
for,   𝛽𝑖 = 0
(4.114)
The  standard  formulation  for  the  twenty  node  solid  element  is  used  with  the  above 
trans-formations.    The  element  is  integrated  with  a  fourteen  point  integration  rule 
[Cook 1974]: 
  1
  1
  1
−1
−1
∫ ∫ ∫ 𝑓 (𝜉  , 𝜂 , 𝜁 )𝑑𝜉𝑑𝜂𝑑𝜁 =
−1
         𝐵6  [𝑓 (−𝑏, 0,0) + 𝑓 (𝑏, 0,0) + 𝑓 (0, −𝑏, 0) + ⋯ + (6 terms)] + 
         𝐶8 [𝑓 (−𝑐, −𝑐, −𝑐) + 𝑓 (𝑐, −𝑐, −𝑐) + 𝑓 (𝑐, 𝑐, −𝑐) + ⋯ + (8 terms)], 
where 
𝐵6 = 0.8864265927977938,
𝐶8 = 0.3351800554016621,
𝑏 = 0.7958224257542215,
𝑐 = 0.7587869106393281.
(4.115)
(4.116)
Solid Elements 
LS-DYNA Theory Manual 
Cook  reports  that  this  rule  has  nearly  the  same  accuracy  as  the  twenty-seven  point 
Gauss  rule,  which  is  very  costly.    The  difference  in  cost  between  eight  point  and 
fourteen point integration, though significant, is necessary to eliminate the zero energy 
modes.
4.10  Fully Integrated Tetrahedron Element With 24 Degrees-
of-Freedom 
The twenty-four degree of freedom tetrahedron element is derived from the ten-
node tetrahedron element; see Figure 4.8, following the same procedure used above for 
the forty-eight degree of freedom brick element [Yunus, Pawlak, and Cook, 1989].  This 
element  has  the  advantage  that  shell  nodes  can  be  shared  with  its  nodes  and  it  is 
compatible  with  the  brick  element  discussed  above.    The  accuracy  of  this  element  is 
relatively good-at least when compared to the constant strain tetrahedron element.  This 
is  illustrated  by  the  bar  impact  example  in  Figure  4.9  which  compares  the  12  and  24 
degree  of  freedom  tetrahedron  elements.    The  12  degree-of-freedom  tetrahedron 
displays severe volumetric locking. 
In  our  implementation  we  have  not  strictly  followed  the  reference.    In  order  to 
prevent locking in applications that involve incompressible behavior, selective reduced 
integration  is  used  with  a  total  of  5  integration  points.    Although  this  is  rather 
expensive, no zero energy modes exist.  We use the same approach in determining the 
rotary mass that is used in the implementation of the shell elements.
LS-DYNA Theory Manual 
Solid Elements 
Figure  4.9.    A  comparison  of  the  12  and  24  degree-of-freedom  tetrahedron 
elements is shown.  The 12 degree-of-freedom tetrahedron element on the top 
displays severe volumetric locking.
Solid Elements 
LS-DYNA Theory Manual 
  Figure 4.10a.  Construction of a hexahedron element with five tetrahedrons. 
  Figure 4. 10b.  Construction of a hexahedron element with six tetrahedrons 
Figures  4.10a  and  4.  10b  show  the  construction  of  a  hexahedron  element  from 
five and six tetrahedron elements, respectively.  When two sides of the adjacent bricks 
made  from  five  tetrahedrons  are  together,  it  is  likely  that  four  unique  triangular 
segments exist.  This creates a problem in LS-PREPOST, which uses the numbering as a 
basis for eliminating interior polygons prior to display.  Consequently, the graphics in 
the  post-processing  phase  can  be  considerably  slower  with  the  degeneration  in Figure 
4.10a.  However, marginally better results may be obtained with five tetrahedrons per 
hexahedron due to a better constraint count.
LS-DYNA Theory Manual 
Solid Elements 
4.11  The Cosserat Point Elements in LS-DYNA 
4.11.1  Introduction 
The  Cosserat  Point  Elements  (CPE)  are  based  on  the  works  by  Jabareen  et.al.[1,2].    In 
contrast  with  a  conventional  approach,  the  CPE  is  treated  as  a  structure  rather  than  a 
continuum.  The kinematic variables of the CPE are characterized by a volume averaged 
deformation  gradient  and  other  measures  of  inhomogeneous  deformations.    The  CPE 
models the response of a simple continuum (not a generalized Cosserat media) and the 
additional  kinematic  degrees  of  freedom  model  physical  modes  of  deformation  of  the 
structure.    Moreover,  the  CPE  uses  a  hyperelastic  constitutive  equation  for  elastic 
response  with  the  strain  energy  of  the  CPE  being  separated  additively  into  a  part 
dependent  on  the  strain  energy  of  the  three-dimensional  material  and  another  strain 
energy associated with inhomogeneous deformations.  Also, for the tetrahedral CPE use 
is  made  of  a  new  measure  of  dilatation  that  stabilizes  hourglass  type  modes  in  large 
deformations.    This  formulation  is  valid  for  large  deformations  and  the  coefficients  in 
the inhomogeneous strain energy are ingeniously determined by comparison with exact 
linear  solutions.    This  ensures  that  CPE  yields  accurate  results  for  elementary 
deformation  modes  in  linear  elasticity.    Moreover,  using  the  average  deformation 
gradient  for  the  response  to  homogeneous  deformations  the  CPE  formulation  can  be 
coupled  with  arbitrary  material  models  in  LS-DYNA.  Still  the  element  is,  due  to  its 
complexity  and  slight  loss  of  generality,  first  and  foremost  recommended  for 
hyperelasticy in implicit analysis. 
Section  4.11.2  through  4.11.8  describes  the  theory  for  the  hexahedral  CPE 
element,  the  tetrahedron  is  based  on  the  same  concepts  except  for  the  volumetric 
correction presented in Section 4.11.5. For more details we refer to [1] and [2].  We end 
with two examples in Sections 4.11.9 and 4.11.10. 
D3
D1
D2
d3
d1
d2
Figure 4.11.  The CPE hexahedron
Solid Elements 
4.11.2  Geometry 
LS-DYNA Theory Manual 
The geometry of the hexahedral CPE element is characterized by the three-dimensional 
directors  𝐃𝑖  and  𝐝𝑖,  𝑖 = 0,1, … ,7,  where  the  formers  are  associated  with  the  reference 
configuration and the latters with the current configuration.  The reciprocal vectors 𝐃𝑖 
and 𝐝𝑖, 𝑖 = 1,2,3, are such that 
𝑗,
𝐝𝑖 ⋅ 𝐝𝑗 = 𝐃𝑖 ⋅ 𝐃𝑗 = 𝛿𝑖
𝑖, 𝑗 = 1, 2, 3,
and we also have that 
The coordinates 𝜃𝑖, 𝑖 = 1,2,3, ranges between 
|𝐃𝑖| = 1,
𝑖 = 1, 2, 3,
(4.11.117)
(4.11.118)
−𝐻/2 ≤ 𝜃1 ≤ 𝐻/2,     − 𝑊/2 ≤ 𝜃2 ≤ 𝑊/2, − 𝐿/2 ≤ 𝜃3 ≤ 𝐿/2, 
(4.11.119)
and the 𝐀 matrix is given such that 
𝐃𝑖 = ∑ 𝐴𝑖
𝑗𝐗𝑗
,    𝐝𝑖 = ∑ 𝐴𝑖
𝑗𝐱𝑗
,
𝑖 = 0, 1, . . . , 7,
(4.11.120)
𝑗=0
𝑗=0
where  𝐗𝑖  and  𝐱𝑖  are  the  nodal  coordinates  in  the  reference  and  current  configuration, 
respectively.    Hence  the  𝐀  matrix  represents  the  mapping  between  the  nodal 
coordinates  and  the  Cosserat  point  directors.    The  reference  position  vector  𝐗  is 
expressed as 
𝐗 = 𝐗(𝜃1, 𝜃2, 𝜃3) = ∑ 𝑁𝑗(𝜃1, 𝜃2, 𝜃3)𝐃𝑗
,
(4.11.121)
𝑗=0
and likewise the current position 𝐱 as 
𝐱 = 𝐱(𝜃1, 𝜃2, 𝜃3) = ∑ 𝑁𝑗(𝜃1, 𝜃2, 𝜃3)𝐝𝑗,
𝑗=0
The shape functions are given as 
𝑁0 = 1,
𝑁4 = 𝜃1𝜃2, 𝑁5 = 𝜃1𝜃3, 𝑁6 = 𝜃2𝜃3, 𝑁7 = 𝜃1𝜃2𝜃3.
𝑁3 = 𝜃3,
𝑁1 = 𝜃1,
𝑁2 = 𝜃2,
(4.11.122)
(4.11.123)
4.11.3  Deformation and strain 
The deformation measures used are 
𝐅 = ∑ 𝐝𝑖 ⊗ 𝐃𝑖
𝑖=1
,    𝛃𝑖 = 𝐅−1𝐝𝑖+3 − 𝐃𝑖+3 (𝑖 = 1,2,3,4), 𝐅̅̅̅̅ = 𝐅 (𝐈 + ∑ 𝛃𝑖 ⊗ 𝐕𝑖
),  (4.11.124)
𝑖=1
where  𝐅̅̅̅̅  is  the  volume  averaged  deformation  gradient  and  thus  represents  the 
inhomogeneous 
homogeneous  deformations  whereas  𝛃𝑖  are  measures  of 
deformations.  As for the 𝐕𝑖 we have 
the
LS-DYNA Theory Manual 
Solid Elements 
𝑉 = 𝐻𝑊𝐿 (𝐃1 × 𝐃2 ⋅ 𝐃3 +
𝐻2
12
𝐃4 × 𝐃5 ⋅ 𝐃1 +
× 𝐃4 ⋅ 𝐃2 +
𝐃6
𝑊2
12
𝐿2
12
𝐃5 × 𝐃6 ⋅ 𝐃3) , 
𝐃2 × 𝐃6) , 
(4.11.125)
𝐕1 = 𝑉−1𝐻𝑊𝐿 (
𝐕2 = 𝑉−1𝐻𝑊𝐿 (
𝐕3 = 𝑉−1𝐻𝑊𝐿 (
𝐕4 = 𝟎, 
𝐻2
12
𝐻2
12
𝑊2
12
𝐃5 × 𝐃1 +
𝐃1 × 𝐃4 +
𝐃4 × 𝐃2 +
𝑊2
12
𝐿2
12
𝐿2
12
𝐃6 × 𝐃3) , 
𝐃3 × 𝐃5) , 
The velocity gradient consistent with 𝐅̅̅̅̅ is given as 
𝐋̅ = 𝐅̅̅̅̅̇𝐅̅̅̅̅−1 = 𝐋 + ∑(𝐝̇
𝑗+3 − 𝐋𝐝𝑗+3) ⊗ 𝐕𝑗
𝐅̅̅̅̅−1,
𝑗=1
(4.11.126)
where 𝐋 = 𝐅̇𝐅−1, which in turn gives the rate –of-deformation and spin tensors as 
̇ =
𝛆̅
(𝐋̅ + 𝐋̅ 𝑇), 𝛚̅̅̅̅̅̅ =
(𝐋̅ − 𝐋̅ 𝑇).
(4.11.127)
4.11.4  Stress and Force 
On the other hand, 
𝐋 = ∑ 𝐝̇
𝑖=1
𝑖 ⊗ 𝐝𝑖
,
(4.11.128)
so we can rewrite 𝐋̅  as 
𝐋̅ = ∑ 𝐝̇
𝑖=1
𝑖 ⊗ 𝐝𝑖
⎜⎛𝐅̅̅̅̅ − ∑ 𝐝𝑗+3 ⊗ 𝐕𝑗
⎝
𝑗=1
⎟⎞ 𝐅̅̅̅̅−1 + ∑ 𝐝̇
⎠
𝑖=1
The Cauchy stress is given by the constitutive law 
or for the hyperelastic case 
𝛔∇ = 𝐟hypo(𝛆̅
̇, . . . ),
𝛔 = 𝐟hyper(𝐅̅̅̅̅, . . . ),
so the nonzero internal force vectors are given as 
𝑖+3 ⊗ 𝐕𝑖
𝐅̅̅̅̅−1. 
(4.11.129)
(4.11.130)
(4.11.131)
Solid Elements 
LS-DYNA Theory Manual 
𝑖 = 𝐽 ̅𝑉𝛔𝐅̅̅̅̅−𝑇
𝐭𝜎
⎜⎛𝐅̅̅̅̅𝑇 − ∑ 𝐕𝑗 ⊗ 𝐝𝑗+3
⎝
𝑗=1
⎟⎞ 𝐝𝑖,
⎠
𝑖+3 = 𝑉𝛔𝐅̅̅̅̅−𝑇𝐕𝑖,
𝐭𝜎
𝑖 = 1, 2, 3. 
(4.11.132)
The first expression above can in turn be rewritten as 
𝑖 =
𝐭𝜎
⎜⎛𝐽 ̅𝑉𝛔 − ∑ 𝐭𝜎
⎝
𝑗=1
𝑗+3 ⊗ 𝐝𝑗+3
⎟⎞ 𝐝𝑖,
⎠
𝑖 = 1, 2, 3.
(4.11.133)
4.11.5  CPE3D10 modification 
For  the  10-noded  tetrahedron,  a  modified  deformation  gradient  is  used  in  the 
constitutive law, given by 
𝐅̃ = (𝐽 ̃
𝐽 ̅⁄ )
1/3
𝐅̅̅̅̅,
meaning it has been modified for the volumetric response.  Here 
This gives a consistent velocity gradient as 
𝐽 ̃ = 𝐽 ̅ + 𝜂𝐽,
𝐋̃ = 𝐋̅ +
⎜⎛𝜂̇ + 𝜂
𝐽 ̃⎝
{⎧𝐽 ̇
⎩{⎨
−
𝐽 ̅
}⎫
𝐽 ̅⎭}⎬
⎟⎞ 𝐈.
⎠
The Cauchy stress is now given by the constitutive law 
𝛔∇ = 𝐟hypo(𝛆̃
̇, … ),
̇ =
𝛆̃
(𝐋̃ + 𝐋̃ 𝑇),
or for the hyperelastic case 
𝛔 = 𝐟hyper(𝐅̃, . . . ),
(4.11.134)
(4.11.135)
(4.11.136)
(4.11.137)
(4.11.138)
and  the  corresponding  internal  force  can  be  identified  through  a  principle  of  virtual 
work 
∑ 𝐭𝜎
𝑖=0
𝑖 ⋅ 𝐝̇
= 𝐽 ̃𝑉𝐋̃ ⋅ 𝛔.
For the hyperelastic special case we have 
𝛔 =
∂Σ
∂𝐽 ̃
𝐈 + 2𝐽 ̃−1 [𝐅̅̅̅̅′
∂Σ
∂𝐂̅′
𝐅̅̅̅̅′𝑇 −
(
∂Σ
∂𝐂̅′
⋅ 𝐂̅′) 𝐈],
and since 
(4.11.139)
(4.11.140)
4-34 (Solid Elements)
LS-DYNA Theory Manual 
Solid Elements 
𝐋̃ = ∑ 𝐝̇
𝑖=1
𝑖 ⊗ 𝐝𝑖
+  
+  
⎟⎞ 𝐅̅̅̅̅−1 + ∑ 𝐝̇
⎠
((𝐝𝑘)
𝑖=1
𝐝̇
𝑗=1
∑ ∑
𝑗=1
𝑘=1
⎜⎛𝐅̅̅̅̅ − ∑ 𝐝𝑗+3 ⊗ 𝐕𝑗
⎝
𝐽 ̃
⎡𝜂
⎢
𝐽 ̃⎣
⎜⎛∑ ∑ 𝐝𝑖 ⋅ 𝐝𝑗+3𝐝̇
⎝
⎡ ∂𝜂
⎢
∂𝑏𝑗
⎣
𝑗=1
𝑖=1
𝑖=1
𝑖 ⋅ 𝐅̅̅̅̅−𝑇𝐕𝑗
−
𝑗+3 − ∑ 𝐝𝑖 ⋅ 𝐝𝑗+3𝐝𝑘 ⋅ 𝐝̇
)
⎤
⎥
⎦
(4.11.141)
∑ 𝐝̇
𝑖=1
𝑖+3 ⋅ 𝐅̅̅̅̅−𝑇𝐕𝑖
⎟⎞
⎠
⎤ 𝐈, 
⎥
⎦
𝑖+3 ⊗ 𝐕𝑖
𝐅̅̅̅̅−1
putting  back  these  expressions  into  the  virtual  work  expression  above  and  adding  the 
hourglass internal forces from below we get the same as in [2].  
4.11.6  Hourglass 
The hourglass resistance is based on a strain energy potential given as 
𝜓 =
𝑉𝜇
12(1 − 𝜈)
∑ ∑ ∑ ∑ 𝑏𝑖
𝑖=1
𝑘=1
𝑗=1
𝑙=1
𝑗𝐵𝑗𝑙
𝑖𝑘𝑏𝑘
,
(4.11.142)
where the inhomogeneous (hourglass) strain quantities are defined as 
𝑗 = 𝛃𝑖 ⋅ 𝐃𝑗,
𝑏𝑖
𝑖 = 1, 2, 3, 4,
𝑗 = 1, 2, 3,
(4.11.143)
and  the  constant  symmetric  matrix  𝐁  contains  geometry  and  constitutive  information 
for  obtaining  accurate  results  for  small  deformations.    Furthermore,  𝜇  represents  the 
shear modulus of the material and 𝜈 is the Poisson’s ratio.  The hourglass force is then 
given as 
⎜⎛∂𝑏𝑗
⎟⎞
∂𝐝𝑖⎠
⎝
Differentiating the strain quantities results in 
= ∑ ∑
𝑗=1
𝑘=1
∂𝜓
∂𝑏𝑗
𝑖 = (
𝐭ℎ
∂𝜓
∂𝐝𝑖
)
,
𝑖 = 0, 1, … ,7. 
(4.11.144)
∂𝑏𝑗
∂𝐝𝑖
∂𝑏𝑗
∂𝐝𝑖+3
= −𝐝𝑖 ⋅ 𝐝𝑗+3(𝐝𝑘)
,
𝑖 = 1, 2, 3
𝑗(𝐝𝑘)
= 𝛿𝑖
,
𝑖 = 1,2,3,4
(4.11.145)
which inserted into the expression for the force yields
Solid Elements 
LS-DYNA Theory Manual 
𝑖 = −
𝐭ℎ
𝑗+3 ⊗ 𝐝𝑗+3
⎜⎛∑ 𝐭ℎ
⎝
𝑗=1
∂𝜓
𝑗 𝐝𝑗
∂𝑏𝑖
𝑖+3 = ∑
𝐭ℎ
𝑗=1
,
𝑖 = 1,2,3,4
⎟⎞ 𝐝𝑖,
⎠
𝑖 = 1,2,3
(4.11.146)
4.11.7  Comparison to Jabareen & Rubin 
Putting the material and hourglass force together yields  
𝐭𝑖 = 𝐭𝜎
𝑖 = 0,1, . . . ,7,
𝑖 ,
𝑖 + 𝐭ℎ
hence 
𝐭𝑖 =
⎜⎛𝐽 ̅𝑉𝛔 − ∑ 𝐭𝑗+3 ⊗ 𝐝𝑗+3
⎝
𝑗=1
𝐭𝑖+3 = 𝐽 ̅𝑉𝛔𝐅̅̅̅̅−T𝐕𝑖 + ∑
𝑗=1
𝑗 𝐝𝑗
∂𝜓
∂𝑏𝑖
⎟⎞ 𝐝𝑖
⎠
𝑖 = 1,2,3
𝑖 = 1,2,3,4
(4.11.147)
(4.11.148)
𝑗 are augmented with the geometry parameters 𝐻,𝑊 and 𝐿, 
In [1], the hourglass strains 𝑏𝑖
whereas  here  we  have  merged  this  information  into  the  constitutive  matrix  𝐁  for  the 
purpose  of  simplifying  the  presentation.    In  [1]  a  hyperelastic  constitutive  law  is 
assumed with a strain energy potential  Σ = Σ(𝐂̅) and the Cauchy stress is then given 
as 
𝛔 = 2𝐽 ̅−1𝐅̅̅̅̅
∂Σ
∂𝐂̅
𝐅̅̅̅̅T.
(4.11.149)
Taking  all  this  into  account,  and  consulting  (2.13-2.14)  in  [1],  the  implemented  CPE 
element in LS-DYNA should be consistent with the theory. 
4.11.8  Nodal formulation 
To be of use in LS-DYNA, the CPE element has to be formulated in terms of the nodal 
variables,  meaning  that  the  internal  forces  that  are  conjugate  to  𝐱̇𝑖,  𝑖 = 0,1, . . . ,7,  with 
respect to internal energy rate are given as 
𝑖𝐭𝑗
𝐟𝑖 = ∑ 𝐴𝑗
𝑗=0
,
𝑖 = 0,1, … ,7.
(4.11.150)
LS-DYNA Theory Manual 
Solid Elements 
Figure  4.11.   Stress profile  for  tip loading in two  directions for various mesh
densities and distortions 
4.11.9  Cantilever Beam Example 
First a mesh distortion test for small deformations where a cantilever beam with various 
mesh  densities  and  distortions  were  simulated.    The  stress  profiles  for  loading  in  two 
directions  are  shown  in  Figure  4.11.  The  tip  displacements  were  monitored  and 
compared  to  the  analytical  solution,  and  the  results  for  the  CPE  element  is  very 
promising  as  is  shown  in  figure  below  and    Table  4.11  when  compared  to  the 
Belytschko-Bindeman and Puso element [3,4]. 
 0.7
 0.6
 0.5
 0.4
 0.3
 0.2
 0.1
 0
CPE
B-B
Puso
 0.2
 0.4
 0.6
Mesh size
 0.8
 1
Figure 4.11.  Mesh convergence rate for different element formulations
Solid Elements 
LS-DYNA Theory Manual 
Cosserat  Belytschko-Bindeman 
1.7% 
0.8% 
0.6% 
0.3% 
0.2% 
0.2% 
0.1% 
0.1% 
0.1% 
0.1% 
61.8% 
46.8% 
40.0% 
39.8% 
33.9% 
27.0% 
24.6% 
22.3% 
19.0% 
15.4% 
Puso 
24.8% 
14.7% 
14.5% 
9.2% 
8.5% 
6.2% 
5.3% 
3.6% 
0.9% 
0.3% 
Table 4.11.  Comparison to analytical solution for tip loading 
4.11.10  Compression Test for Rubber Example 
The second example is a plane strain deformation of an incompressible rubber block on 
a frictionless surface when partially loaded by a rigid plate.  The block is modeled with 
quadratic  tetrahedrons  and  a  large  deformation  formulation  applies.    Five  different 
mesh topologies are investigated for two different element formulations (CPE and  full 
integration) where the orientation of the tetrahedral elements is different in each mesh 
whereas  the  mesh  density  is  kept  constant.    The  outer  edges  of  the  block  for  the 
different meshes are depicted in the figure above and indicate once again that the CPE 
element formulation is relatively insensitive to the mesh. 
Figure 4.11.  Insensitivity illustration of the 10-noded CPE tetrahedron 
4.11.11  References 
[1]M.  Jabareen  and  M.B.  Rubin,  A  Generalized  Cosserat  Point  Element  (CPE)  for 
Isotropic Nonlinear Elastic Materials including Irregular 3-D Brick and Thin 
Structures, J. Mech.  Mat.  Struct.  3-8, pp.  1465-1498, 2008. 
[2]M.  Jabareen,  E.  Hanukah  and  M.B.  Rubin,  A  Ten  Node  Tetrahedral  Cosserat  Point 
Element (CPE) for Nonlinear Isotropic Elastic Materials.  Comput Mech 52, 
pp 257-285, 2013.
LS-DYNA Theory Manual 
Solid Elements 
Figure 4.11.  The contour S encloses an area A. 
[3]M.A.  Puso,  A  Highly  Efficient  Enhanced  Assumed  Strain  Physically  Stabilized 
Hexahedral Element, In.  J. Num.  Methods.  Eng 49-8, pp.  1029-1064, 2000. 
[4]T.  Belytschko  and  L.P.  Bindeman  ,  Assumed  Strain  Stabilization  of  the  Eight  Node 
Hexahedral Element, Comp.  Methods Appl.  Mech.  Eng.  105-2, pp.  225-
260, 1993.
4.12  Integral Difference Scheme as Basis For 2D Solids 
Two dimensional solid element in LS-DYNA include: 
•  Plane stress 2D element 
•  Plane strain 2D shell element 
•  Axisymmetric 2D Petrov-Galerkin (area weighted) element 
•  Axisymmetric 2D Galerkin (volume weighted) element 
These elements have their origins in the integral difference method of Noh [1964] which 
is also used the HEMP code developed by Wilkins [1964, 1969].  In LS-DYNA, both two 
dimensional  planar  and  axisymmetric  geometries  are  defined  in  the  𝑥𝑦  plane.    In 
axisymmetric geometry, however, the 𝑥 axis corresponds to the radial direction and the 
𝑦  axis  becomes  the  axis  of  symmetry.    The  integral  difference  method  defines  the 
components  of  the  gradient  of  a  function  𝐹  in  terms  of  the  line  integral  about  the 
contour 𝑆 which encloses the area 𝐴: 
∂𝐹
∂𝑥
∂𝐹
∂𝑦
= lim
A→0
= lim
A→0
∫ 𝐹(𝐧̂ ⋅ 𝐱̂)𝑑𝑆
|A|
∫ 𝐹(𝐧̂ ⋅ 𝐲̂)𝑑𝑆
. 
, 
|A|
(4.151)
Here, 𝐧̂ is the normal vector to 𝑆 and 𝐱̂ and 𝐲̂ are unit vectors in the x and y directions, 
respectively.  See Figure 4.11.
Solid Elements 
LS-DYNA Theory Manual 
strain rates
nodal forces
Figure  4.12.    Strain  rates  are  element  centered  and  nodal  forces  are  node 
centered. 
In this approach the velocity gradients which define the strain rates are element 
centered, and the velocities and nodal forces are node centered.  See Figure 4.12.  Noting 
that the normal vector 𝐧̂ is defined as: 
∂𝑦
∂𝑆
and referring to Figure 4.13, we can expand the numerator in equation (4.64): 
∂𝑥
∂𝑆
𝐧̂ =
𝐱̂ +
𝐲̂,
∫ 𝐹(n̂ ⋅ x̂)𝑑𝑆
= ∫ 𝐹
∂𝑦
∂𝑆
𝑑𝑆 
= 𝐹23(𝑦3 − 𝑦2) + 𝐹34(𝑦4 − 𝑦3) + 𝐹41(𝑦1 − 𝑦4) + 𝐹12(𝑦2 − 𝑦1), 
where 𝐹𝑖𝑗 = (𝐹𝑖 + 𝐹𝑗)/2. 
(4.152)
(4.153)
Therefore,  letting  𝐴  again  be  the  enclosed  area,  the  following  expressions  are 
obtained: 
∂𝐹
∂𝑥
=
=
𝐹23(𝑦3 − 𝑦2) + 𝐹34(𝑦4 − 𝑦3) + 𝐹41(𝑦1 − 𝑦4) + 𝐹12(𝑦2 − 𝑦1)
(𝐹2 − 𝐹4)(𝑦3 − 𝑦1) + (𝑦2 − 𝑦4)(𝐹3 − 𝐹1)
.
2𝐴
Hence, the strain rates in the x and y directions become: 
∂𝐹
∂𝑥
=
=
𝐹23(𝑦3 − 𝑦2) + 𝐹34(𝑦4 − 𝑦3) + 𝐹41(𝑦1 − 𝑦4) + 𝐹12(𝑦2 − 𝑦1)
(𝐹2 − 𝐹4)(𝑦3 − 𝑦1) + (𝑦2 − 𝑦4)(𝐹3 − 𝐹1)
,
2𝐴
(4.154)
(4.155)
LS-DYNA Theory Manual 
Solid Elements 
1 
Figure 4.13.  Element numbering. 
and 
𝜀𝑦𝑦 =
∂𝑦̇
∂𝑦
=
(𝑦̇2 − 𝑦̇4)(𝑥3 − 𝑥1) + (𝑥2 − 𝑥4)(𝑦̇3 − 𝑦̇1)
2𝐴
.
The shear strain rate is given by: 
𝜀𝑥𝑦 =
(
∂𝑦̇
∂𝑥
+
∂𝑥̇
∂𝑦
),
where  
∂𝑦̇
∂𝑥
∂𝑥̇
∂𝑦
=
=
(𝑦̇2 − 𝑦̇4)(𝑦3 − 𝑦1) + (𝑦2 − 𝑦4)(𝑦̇3 − 𝑦̇1)
2𝐴
(𝑥̇2 − 𝑥̇4)(𝑥3 − 𝑥1) + (𝑥2 − 𝑥4)(𝑥̇3 − 𝑥̇1)
2𝐴
.
,
(4.156)
(4.157)
(4.158)
The  zero  energy  modes,  called  hourglass  modes,  as  in  the  three  dimensional 
solid elements, can be a significant problem.  Consider the velocity field given by: 𝑥̇3 =
𝑥̇1, 𝑥̇2 = 𝑥̇4, 𝑦̇3 = 𝑦̇1, and 𝑦̇2 = 𝑦̇4.  As can be observed from Equations (4.97) and (4.98), 
𝜀𝑥𝑥 = 𝜀𝑦𝑦 = 𝜀𝑥𝑦 = 0 and the element "hourglasses" irrespective of the element geometry.  
In the two-dimensional case, two modes exist versus twelve in three dimensions.  The 
hourglass  treatment  for  these  modes  is  identical  to  the  approach  used  for  the  shell 
elements, which are discussed later. 
In two-dimensional planar geometries for plane stress and plane strain, the finite 
element  method  and  the  integral  finite  difference  method  are  identical.    The  velocity 
strains are computed for the finite element method from the equation: 
𝛆̇ = 𝐁𝐯,
(4.159)
where  𝛆̇  is  the  velocity  strain  vector,  B  is  the  strain  displacement  matrix,  and  𝐯  is  the 
nodal velocity vector.  Equation (4.100a) exactly computes the same velocity strains as 
the integral difference method if  
LS-DYNA Draft 
𝐁 = 𝐁(𝑠, 𝑡)|𝑠=𝑡=0.
Solid Elements 
LS-DYNA Theory Manual 
IV
III
II
 Figure 4.14.  The finite difference stencil for computing nodal forces is shown.
The  update  of  the  nodal  forces  also  turns  out  to  be  identical.    The  momentum 
equations in two-dimensional planar problems are given by  
(
(
∂𝜎𝑥𝑥
∂𝑥
∂𝜎𝑥𝑦
∂𝑥
+
+
∂𝜎𝑥𝑦
∂𝑦
∂𝜎𝑦𝑦
∂𝑦
) = 𝑥̈,
) = 𝑦̈.
(4.161)
Referring to Figure 4.14, the integral difference method gives Equation (4.113): 
∂𝜎𝑥𝑥
∂𝑥
=
𝜎𝑥𝑥1(𝑦𝐼 − 𝑦𝐼𝑉) + 𝜎𝑥𝑥2(𝑦𝐼𝐼 − 𝑦𝐼) + 𝜎𝑥𝑥3(𝑦𝐼𝐼𝐼 − 𝑦𝐼𝐼) + 𝜎𝑥𝑥4(𝑦𝐼𝑉 − 𝑦𝐼𝐼𝐼)
(𝜌1𝐴1 + 𝜌2𝐴2 + 𝜌3𝐴3 + 𝜌4𝐴4)
. 
(4.162)
An  element  wise  assembly  of  the  discretized  finite  difference  equations  is 
possible leading to a finite element like finite difference program.  This approach is used 
in the DYNA2D program by Hallquist [1980]. 
In  axisymmetric  geometries  additional  terms  arise  that  do  not  appear  in  planar 
problems: 
(
∂𝜎𝑥𝑥
∂𝑥
(
+
∂𝜎𝑥𝑦
∂𝑦
∂𝜎𝑥𝑦
∂𝑥
+
+
𝜎𝑥𝑥 − 𝜎𝜃𝜃
∂𝜎𝑥𝜃
+
∂𝜎𝑦𝑦
∂𝑦
) = 𝑥̈, 
) = 𝑦̈, 
(4.163)
where again note that 𝑦 is the axis of symmetry and 𝑥 is the radial direction.  The only 
difference  between  finite  element  approach  and  the  finite  difference  method  is  in  the 
treatment of the terms, which arise from the assumption of axisymmetry.  In the finite 
difference method the radial acceleration is found from the calculation:
LS-DYNA Theory Manual 
Solid Elements 
𝑥̈ =
𝜎𝑥𝑥1(𝑦𝐼 − 𝑦𝐼𝑉) + 𝜎𝑥𝑥2(𝑦𝐼𝐼 − 𝑦𝐼) + 𝜎𝑥𝑥3(𝑦𝐼𝐼𝐼 − 𝑦𝐼𝐼) + 𝜎𝑥𝑥4(𝑦𝐼𝑉 − 𝑦𝐼𝐼𝐼)
[
(𝜌1𝐴1 + 𝜌2𝐴2 + 𝜌3𝐴3 + 𝜌4𝐴4)
−
𝜎𝑥𝑦1(𝑥𝐼 − 𝑥𝐼𝑉) + 𝜎𝑥𝑦2(𝑥𝐼𝐼 − 𝑥𝐼) + 𝜎𝑥𝑦3(𝑥𝐼𝐼𝐼 − 𝑥𝐼𝐼) + 𝜎𝑥𝑦4(𝑥𝐼𝑉 − 𝑥𝐼𝐼𝐼)
(𝜌1𝐴1 + 𝜌2𝐴2 + 𝜌3𝐴3 + 𝜌4𝐴4)
] + 𝛽,
where 𝛽𝑓𝑒 is found by a summation over the four surrounding elements: 
𝛽 =
∑ [
𝑖=1
𝜎𝑥𝑥𝑖 − 𝜎𝜃𝜃𝑖
(𝜌𝑥)𝑖
]
.
(4.164)
(4.165)
𝑥𝑖 is the centroid of the ith element defined as the ratio of its volume 𝑉𝑖 and area 𝐴𝑖: 
𝑉𝑖
𝐴𝑖
𝑥𝑖 =
,
(4.166)
𝜎𝜃𝜃𝑖 is the hoop stress, and 𝜌𝑖 is the current density. 
When  applying  the  Petrov-Galerkin  finite  element  approach,  the  weighting 
functions are divided by the radius, 𝑟: 
∫
𝛟T(∇ ⋅ 𝛔 + 𝐛 − 𝜌𝐮̈)𝑑𝑉 = ∫ 𝛟T(∇ ⋅ 𝛔 + 𝐛 − 𝜌𝐮̈)𝑑𝐴 = 0, 
(4.167)
where the integration is over the current geometry.  This is sometimes referred to as the 
"Area  Galerkin"  method.    This  approach  leads  to  a  time  dependent  mass  vector.    LS-
DYNA  also  has  an  optional  Galerkin  axisymmetric  element,  which  leads  to  a  time 
independent mass vector.  For structural analysis problems where pressures are low the 
Galerkin approach works best, but in problems of hydrodynamics where pressures are 
a  large  fraction  of  the  elastic  modulus,  the  Petrov-Galerkin  approach  is  superior  since 
the behavior along the axis of symmetry is correct. 
The  Petrov-Galerkin  approach  leads  to  equations  similar  to  finite  differences.  
The radial acceleration is given by. 
𝑥̈ =
𝜎𝑥𝑥1(𝑦𝐼 − 𝑦𝐼𝑉) + 𝜎𝑥𝑥2(𝑦𝐼𝐼 − 𝑦𝐼) + 𝜎𝑥𝑥3(𝑦𝐼𝐼𝐼 − 𝑦𝐼𝐼) + 𝜎𝑥𝑥4(𝑦𝐼𝑉 − 𝑦𝐼𝐼𝐼)
[
(𝜌1𝐴1 + 𝜌2𝐴2 + 𝜌3𝐴3 + 𝜌4𝐴4)
−
𝜎𝑥𝑦1(𝑥𝐼 − 𝑥𝐼𝑉) + 𝜎𝑥𝑦2(𝑥𝐼𝐼 − 𝑥𝐼) + 𝜎𝑥𝑦3(𝑥𝐼𝐼𝐼 − 𝑥𝐼𝐼) + 𝜎𝑥𝑦4(𝑥𝐼𝑉 − 𝑥𝐼𝐼𝐼)
(𝜌1𝐴1 + 𝜌2𝐴2 + 𝜌3𝐴3 + 𝜌4𝐴4)
] + 𝛽𝑓𝑒,
where 𝛽𝑓𝑒 is now area weighted. 
𝛽𝑓𝑒 =
4(𝜌1𝐴1 + 𝜌2𝐴2 + 𝜌3𝐴3 + 𝜌4𝐴4)
∑
𝑖=1
(𝜎𝑥𝑥𝑖 − 𝜎𝜃𝜃𝑖)𝐴𝑖
⎢⎡
𝑥𝑖
⎣
⎥⎤
. 
⎦
(4.168)
(4.169)
In  LS-DYNA,  the  two-dimensional  solid  elements  share  the  same  constitutive 
subroutines  with  the  three-dimensional  elements.    The  plane  stress  element  calls  the 
plane stress constitutive models for shells.  Similarly, the plane strain and axisymmetric 
elements  call  the  full  three-dimensional  constitutive  models  for  solid  elements.    Slight
Solid Elements 
LS-DYNA Theory Manual 
overheads exists since the strain rate components 𝜀̇𝑦𝑧 and 𝜀̇𝑧𝑥 are set to zero in the two-
dimensional  case  prior  to  updating  the  six  stress  component;  consequently,  the 
additional  work  is  related  to  having  six  stresses  whereas  only  four  are  needed.    A 
slowdown of LS-DYNA compared with DYNA2D of fifteen percent has been observed; 
however,  some  of  the  added  cost  is  due  to  the  internal  and  hourglass  energy 
calculations, which were not done in DYNA2D.
4.12.1  Rezoning With 2D Solid Elements 
Lagrangian  solution  techniques  generally  function  well  for  problems  when 
element distortions are moderate.  When distortions become excessive or when material 
breaks  up,  i.e.,  simply  connected  regions  become  multi-connected,  these  codes  break 
down,  and  an  Eulerian  approach  is  a  necessity.    Between  these  two  extremes, 
applications  exist  for  which  either  approach  may  be  appropriate  but  Lagrangian 
techniques  are  usually  preferred  for  speed  and  accuracy.    Rezoning  may  be  used  to 
extend the domain of application for Lagrangian codes. 
Rezoning capability was added to DYNA2D in 1980 and to LS-DYNA in version 
940.  In the current implementation the rezoning can be done interactively and used to 
relocate  the  nodal  locations  within  and  on  the  boundary  of  parts.    This  method  is 
sometimes referred to as r-adaptive. 
The rezoning is accomplished in three steps listed below: 
1.  Generate nodal values for all variables to be remapped 
2.  Rezone  one  or  more  materials  either  interactively  or  automatically  with 
command file. 
3. 
Initialize  remeshed  regions  by  interpolating  from  nodal  point  values  of  old 
mesh. 
In the first step each variable is approximated globally by a summation over the 
number of nodal points 𝑛: 
𝑔(𝑟, 𝑧) = ∑ 𝑔𝑖Φ𝑖(𝑟, 𝑧)
𝑖=1
,
(4.170)
where 
Φ𝑖 = set of piecewise continuous global basis functions 
𝑔𝑖 = nodal point values 
Given  a  variable  to  be  remapped  h(𝑟, 𝑧),  a  least  squares  best  fit  is  found  by 
minimizing the functional 
4-44 (Solid Elements) 
Π = ∫(𝑔 − ℎ)2𝑑𝐴,
LS-DYNA Theory Manual 
Solid Elements 
Ajusted
node
Figure 4.15.  The stencil used to relax an interior nodal point. 
i.e., 
𝑑Π
𝑑𝑔𝑖
= 0,
𝑖 = 1, 2, … , 𝑛.
This yields the set of matrix equations 
𝐌𝐠 = 𝐟,
where 
𝐌 = ∑ 𝐌𝑒 = ∑ ∫ 𝚽𝚽T𝑑𝐴
,
𝐟 = ∑ 𝐟𝑒 = ∑ ∫ ℎ𝚽𝑑𝐴
.
Lumping the mass makes the calculation of 𝑔 trivial 
,
𝑀𝑖 = ∑ 𝑀𝑖𝑗
𝑓𝑖
𝑀𝑖
𝑔𝑖 =
.
(4.172)
(4.173)
(4.174)
(4.175)
In step 2, the interactive rezoning phase permits: 
•  Plotting of solution at current time 
•  Deletion of elements and slidelines 
•  Boundary modifications via dekinks, respacing nodes, etc. 
•  Mesh smoothing 
A large number of interactive commands are available and are described in the 
Help package.  Current results can be displayed by 
•  Color fringes 
•  Contour lines 
•  Vectors plots
Solid Elements 
LS-DYNA Theory Manual 
old mesh
new mesh
Figure 4.16.  A four point Gauss quadrature rule over the new element is used
to determine the new element centered value. 
•  Principal stress lines 
•  Deformed meshes and material outlines 
•  Profile plots 
•  Reaction forces 
•  Interface pressures along 2D contact interfaces 
Three methods are available for smoothing: 
•  Equipotential 
•  Isoparametric 
•  Combination of equipotential and isoparametric. 
In  applying  the  relaxation,  the  new  nodal  positions  are  found  and  given  by  Equation 
(1.176) 
𝑥 =
𝑦 =
∑ 𝜉𝑖𝑥𝑖
𝑖=1
∑ 𝜉𝑖
𝑖=1
∑ 𝜉𝑖𝑦𝑖
𝑖=1
∑ 𝜉𝑖
𝑖=1
, 
, 
(4.176)
where the nodal positions relative to the node being moved are shown in the sketch in 
Figure 4.15.
LS-DYNA Theory Manual 
Solid Elements 
g3
g2
g4
g1
Figure 4.17.  A four point Gauss quadrature rule over the new element is used
to determine the new element centered value. 
The weights, 𝜉𝑖, for equipotential smoothing are 
𝜉1 = 𝜉5 =
[(𝑥7 − 𝑥3)2 + (𝑦7 − 𝑦3)2], 
𝜉4 = 𝜉8 = −𝜉2, 
𝜉2 = 𝜉6 =
𝜉3 = 𝜉7 =
and are given by 
[(𝑥1 − 𝑥5)(𝑥7 − 𝑥3) + (𝑦1 − 𝑦5)(𝑦7 − 𝑦3)], 
[(𝑥1 − 𝑥5)2 + (𝑦1 − 𝑦5)2], 
𝜉1 = 𝜉3 = 𝜉5 = 𝜉7 = .50,
𝜉2 = 𝜉4 = 𝜉6 = 𝜉8 = −.25,
(4.177a)
(4.177b)
(4.177c)
(4.177d)
(4.178)
for  isoparametric  smoothing.    Since  logical  regularity  is  not  assumed  in  the  mesh,  we 
construct  the  nodal  stencil  for  each  interior  node  and  then  relax  it.    The  nodes  are 
iteratively  moved  until  convergence  is  obtained.    In  Chapter  14  of  this  manual,  the 
smoothing procedures are discussed for three-dimensional applications. 
The new element centered values, ℎ∗, computed in Equation (1.179) are found by 
a 4 point Gauss Quadrature as illustrated in Figure 4.16. 
ℎ∗ =
∫ 𝑔𝑑𝐴
∫ 𝑑𝐴
.
(4.179)
The  Gauss  point  values  are  interpolated  from  the  nodal  values  according  to  Equation 
(1.180).  This is also illustrated by Figure 4.17. 
𝑔𝑎 = ∑ 𝜙𝑖 (𝑠𝑎, 𝑡𝑎)𝑔𝑖.
(4.180)
LS-DYNA Theory Manual 
Cohesive Elements 
5    
Cohesive Elements 
The cohesive elements are used for modelling cohesive interfaces between faces of solid 
elements (types 19 and 21), faces of shell elements (types 20 and 22) and edges of shell 
elements (type ±29), typically for treating delamination. 
Element 19 
𝒒3 
Element 20
𝒒1 
𝑛1 
𝑚1 
𝑛4 
𝑚4 
𝑛2 
𝑚2 
𝑛3
𝑚3
𝒒2
𝒒1
𝑛1
𝑚1
𝒒3 
𝑛4 
𝑛2
𝑚4 
𝑛3
𝑚2 
𝑚3
𝒒2
Element ±29 
𝑡 
𝒒3
𝒒1 
𝑛4 
𝑛1 
𝑚4 
𝑚1 
𝑛3 
𝑛2 
𝑚3 
𝑚2 
𝒒2
Cohesive layer
𝒙t
𝒒1
𝒒3 
𝒒2
𝒙b
Figure 5.1.  Illustration of cohesive elements 19, 20 and ±29 
As  a  comparison  to  other  elements,  the  cohesive  “strain”  is  the  separation  distance 
(length)  between  the  two  surfaces,  and  the  cohesive  stress  (force  per  area)  is  its
Cohesive Elements 
LS-DYNA Theory Manual 
conjugate  with  respect  to  the  energy  surface  density  (energy  per  area).    Cohesive 
elements 21 and 22 are pentahedral versions of elements 19 and 20, respectively, where 
the top and bottom surface are triangles.  These elements are not treated here per se, but 
the only difference is that the iso-parametric interpolation functions change. 
5.1  Kinematics 
For this presentation we refer to Figure 5.1 for an illustration. Let 
be the separation of the cohesive layer in the local system, where 
𝒅 = 𝑸𝑻 (𝒙𝑡 − 𝒙𝑏) − 𝒅0,
𝑸 = [𝒒1 𝒒2 𝒒3],
(5.1)
(5.2)
is  the  local  coordinate  system  and  𝒙𝑡  and  𝒙𝑏  are  global  coordinates  on  the  top  and 
bottom  surfaces  for  a  given  iso-parametric  coordinate  (𝜉 , 𝜂).  The  distance  vector  𝒅0 
represents the initial gap for cases where the cohesive interface has a nonzero thickness, 
so 𝒅 = 𝟎 initially.  
For  cohesive  element  19  the  separation  is  given  directly  from  the  solid  element 
geometries (sum over i) 
where 
and  
𝒙𝑡 = 𝒙𝑖
𝑛𝑁𝑖(𝜉 , 𝜂),
𝒙𝑏 = 𝒙𝑖
𝑚𝑁𝑖(𝜉 , 𝜂),
𝑁𝑖(𝜉 , 𝜂) =
(1 + 𝜉 𝑖𝜉 )(1 + 𝜂𝑖𝜂),
𝜉 ∗ = [−1, 1, 1, −1],
𝜂∗ = [−1, −1, 1, 1], 
(5.3)
(5.4)
(5.5)
are the in-plane shape functions.  From here and onwards, superscripts n and m denote 
𝑚 are the nodal coordinates 
the top and bottom surfaces, respectively, and thus 𝒙𝑖
associated with the two surfaces.  
For  cohesive  elements  20  and  ±29,  the  separation  𝒅  is  updated  using  an  incremental 
formulation and we have 
𝑛 and 𝒙𝑖
𝒅 ̇= 𝑸𝑇(𝒙̇𝑡 − 𝒙̇𝑏) + 𝑸̇𝑇𝑸𝒅.
(5.6)
Furthermore, for cohesive element 20 we have (sum over i)
LS-DYNA Theory Manual 
Cohesive Elements 
𝒙̇𝑡 = {𝒙̇𝑖
𝑛 −
𝒙̇𝑏 = {𝒙̇𝑖
𝑚 +
𝝎𝑖
𝑛 × 𝒏𝑡} 𝑁𝑖(𝜉 , 𝜂),
𝝎𝑖
𝑚 × 𝒏𝑏} 𝑁𝑖(𝜉 , 𝜂),
(5.7)
where  the  thicknesses  of  the  two  shells  adjacent  to  the  cohesive  layer  are  denoted  t, 
currently assumed to be the same for the both.  In these equations, 𝒏𝑡 and 𝒏𝑏 are the top 
and bottom shell normal, initially equal to 𝒒3 but they may evolve independently with 
time. For cohesive element ±29 we instead have 
𝒙̇𝑡 = {𝒙̇1
𝑛 + 𝜉
𝑛 × 𝒏𝑡}
𝐱̇𝑏 = {𝐱̇4
𝑚 + 𝜉
𝑚 × 𝐧𝑏}
𝝎1
𝑚    and  𝝎𝑖
𝝎4
1 − 𝜂
1 − 𝜂
+ {𝒙̇2
𝑛 + 𝜉
+ {𝐱̇3
𝑚 + 𝜉
𝝎2
𝑛 × 𝒏𝑡}
𝝎3
𝑚 × 𝐧𝑏}
, 
1 + 𝜂
1 + 𝜂
(5.8)
. 
𝑛  denote  nodal rotational  velocities,  and  also  note that 
In  these  expressions  𝝎𝑖
for  evaluation  the  velocities  of  𝒙𝑡  and  𝒙𝑏  we  assume  that  the  fiber  pointing  from 
assumed mid layer coincides with that of the coordinate axes.  This is in analogy to how 
the  Belytschko-Tsay  element  is  treating  the  fiber  vectors  and  presumably  enhances 
robustness  of  the  elements.    Note  also  that  the  shell  normal  are  in  this  case  initially 
equal to 𝒒1. 
For the local coordinate system, cohesive elements 19 and 20 evaluate this according to 
the invariant node numbering approach for shells using the mid layer node coordinates 
𝒙̅𝑖 =
𝑛 + 𝒙𝑖
𝒙𝑖
, 𝑖 = 1,2,3,4,
𝒆1 =
𝒆2 =
𝒙̅3 − 𝒙̅1
∣𝒙̅3 − 𝒙̅1∣
𝒙̅4 − 𝒙̅2
|𝒙̅4 − 𝒙̅2|
,
,
𝒒1 = −
𝒒2 =
,
𝒆1 + 𝒆2
|𝒆1 + 𝒆2|
𝒆1 − 𝒆2
|𝒆1 − 𝒆2|
,
as follows.  First let 
and then 
followed by 
𝒒3 = 𝒒1 × 𝒒2.
Cohesive element +29 starts by computing 
𝑛 + 𝒙3
𝒙2
𝑛 + 𝒙3
∣𝒙2
𝒒2 =
𝑚 − 𝒙1
𝑚 − 𝒙1
𝑛 − 𝒙4
𝑚∣
𝑛 − 𝒙4
,
(5.9)
(5.10)
(5.11)
(5.12)
(5.13)
Cohesive Elements 
LS-DYNA Theory Manual 
followed by 
and 
𝒒 = 𝒙4
𝑛 + 𝒙3
𝑛 − 𝒙1
𝑚,
𝑚 − 𝒙2
𝒒3 =
𝒒 − 𝒒2𝒒𝑇𝒒2
|𝒒 − 𝒒2𝒒𝑇𝒒2|
,
𝒒1 = 𝒒2 × 𝒒3.
Cohesive element -29 starts by computing 
𝑛 + 𝒙3
𝒙2
𝑛 + 𝒙3
∣𝒙2
𝒒2 =
𝑚 − 𝒙1
𝑚 − 𝒙1
𝑛 − 𝒙4
𝑚∣
𝑛 − 𝒙4
,
followed by 
𝒒 =
(
and 
(𝒙3
∣(𝒙3
𝑛 − 𝒙1
𝑛 − 𝒙1
𝑛) × (𝒙4
𝑛) × (𝒙4
𝑛)
𝑛 − 𝒙2
𝑛)∣
𝑛 − 𝒙2
+
(𝒙3
∣(𝒙3
𝑚 − 𝒙1
𝑚 − 𝒙1
𝑚) × (𝒙4
𝑚) × (𝒙4
𝑚 − 𝒙2
𝑚 − 𝒙2
𝑚)
𝑚)∣
𝒒1 =
𝒒 − 𝒒2𝒒𝑇𝒒2
|𝒒 − 𝒒2𝒒𝑇𝒒2|
,
𝒒3 = 𝒒1 × 𝒒2.
(5.14)
(5.15)
(5.16)
(5.17)
), 
(5.18)
(5.19)
(5.20)
Thus, in pure out-of-plane shear, type +29 will initially have pure tangential traction in 
the  𝑞1-direction,  that  turns  into  a  normal  traction  in  the  𝑞3-direction,  as  the  separation 
increases.  Element type -29, however, will only have tangential traction in this case. 
5.2  Constitutive law 
The  cohesive  constitutive  law  amounts  to  determine  the  normal  and  shear  stress, 
expressed  here  as  the  stress  vector  𝝈,  as  function  of  the  separation  vector  𝒅,  𝝈 =
𝝈(𝒅, … ). The typical appearance of each component of this vector is illustrated in Figure 
5.2.,  the  interface  behaves  elastically  up  to  a  critical  separation  distance  𝑑𝑒  and  peak 
stress 𝜎𝑒 after which damage commences.  The interface is damaged and failure occur at 
a certain critical separation distance 𝑑𝑐, the unloading is typically elastic as indicated by 
the dashed arrow.  
For  detailed  information  on  individual  cohesive  constitutive  laws  we  refer  to  the 
materials section.
LS-DYNA Theory Manual 
Cohesive Elements 
𝜎 
𝜎𝑒 
𝑑𝑒 
𝑑𝑐
𝑑 
Figure 5.2.Common stress versus separation for a cohesive interface 
5.3  Nodal forces 
The principle of virtual work states that (sum over i) 
= {𝒙̇𝑖
𝑛}𝑇𝒇𝑖
𝑚}𝑇𝒇𝑖
𝑚}𝑇𝒓𝑖
𝑚 + {𝒙̇𝑖
𝑛 + {𝝎𝑖
𝑚 + {𝝎𝑖
𝑗 and 𝒓𝑖
∫ 𝒅 ̇𝑇𝝈𝑑𝐴
𝑗 is the nodal force and moment for node i on element j, respectively. The 
where 𝒇𝑖
area A represents the cohesive mid layer spanned by the iso-parametric representation 
and  this  is  used  to  identify  the  nodal  forces  and  moments.    In  the  following  we  work 
out  the  details  for  cohesive  element  ±29.  Cohesive  elements  19  and  20  are  treated 
analogous. 
Using Equation (5.6) we also have 
𝑛}𝑇𝒓𝑖
𝑛, 
(5.21)
∫ 𝐝̇𝑇𝛔𝑑𝐴
𝑇𝐐𝛔𝑑𝐴
= ∫ 𝐱̇𝑡
𝑇𝐐𝛔𝑑𝐴
− ∫ 𝐱̇𝑏
− ∫ 𝐝𝑇𝐐̇ 𝑇𝐐𝛔𝑑𝐴
, 
(5.22)
and before continuing we rewrite (5.8) as 
− {𝝎1
𝑛}𝑇𝑹𝑡
𝑇 = {𝒙̇1
𝒙̇𝑡
where 𝑹∗ is the linear operator defined by 
𝑛}𝑇 1 − 𝜂
𝑚}𝑇 1 − 𝜂
𝑇 1 − 𝜂
𝑇 1 − 𝜂
𝑇 = {𝒙̇4
𝒙̇𝑏
𝑚}𝑇𝑹𝑏
− {𝝎4
+ {𝒙̇2
+ {𝒙̇3
𝑛}𝑇 1 + 𝜂
𝑚}𝑇 1 + 𝜂
− {𝝎2
𝑛}𝑇𝑹𝑡
− {𝝎3
𝑚}𝑇𝑹𝑏
𝑇 1 + 𝜂
𝑇 1 + 𝜂
, 
and insert this into the right of (5.22) which after some simplifications gives 
𝑹∗𝝎 = 𝒏∗ × 𝝎
(5.23)
, 
(5.24)
Cohesive Elements 
LS-DYNA Theory Manual 
∫ 𝒅 ̇𝑇𝝈𝑑𝐴
= − ∫ 𝒅𝑇𝑸̇𝑇𝑸𝝈𝑑𝐴
+{𝐱̇1
𝑛}𝑇 ∫ (
1 − 𝜂
) 𝐐𝛔𝑑𝐴
+ {𝝎1
𝑛}𝑇 ∫ (−
1 − 𝜂
) 𝐑𝑡
𝑇𝐐𝛔𝑑𝐴
+{𝒙̇2
𝑛}𝑇 ∫ (
1 + 𝜂
) 𝑸𝝈𝑑𝐴
+ {𝝎2
𝑛}𝑇 ∫ (−
1 + 𝜂
) 𝑹𝑡
𝑇𝑸𝝈𝑑𝐴
(5.25)
+{𝒙̇4
𝑚}𝑇 ∫ (−
1 − 𝜂
) 𝑸𝝈𝑑𝐴
+ {𝝎4
𝑚}𝑇 ∫ (
1 − 𝜂
) 𝑹𝑏
𝑇𝑸𝝈𝑑𝐴
+{𝒙̇3
𝑚}𝑇 ∫ (−
1 + 𝜂
) 𝑸𝝈𝑑𝐴
+ {𝝎3
𝑚}𝑇 ∫ (
1 + 𝜂
) 𝑹𝑏
𝑇𝑸𝝈𝑑𝐴
. 
If  the  first  term  on  the  right  hand  side  of  (5.25)  is  neglected  we  can,  using  (5.21)  and 
(5.25), identify the nonzero nodal forces and moments 
𝑛 = ∫ (
𝒇1
1 − 𝜂
𝑛 = ∫ (
𝒇2
1 + 𝜂
) 𝑸𝝈𝑑𝐴,
𝑛 = −
𝒓1
) 𝑸𝝈𝑑𝐴,
𝑛 = −
𝒓2
1 − 𝜂
∫ (
1 + 𝜂
∫ (
𝜉 ) 𝑹𝑡
𝑇𝑸𝝈𝑑𝐴,
𝜉 ) 𝑹𝑡
𝑇𝑸𝝈𝑑𝐴,
(5.26)
𝑚 = −𝒇2
𝒇3
𝑛, 𝒓3
𝑚 =
𝑚 = −𝒇1
𝒇4
𝑛, 𝒓4
𝑚 =
1 + 𝜂
∫ (
1 − 𝜂
∫ (
𝜉 ) 𝑹𝑏
𝑇𝑸𝝈𝑑𝐴,
𝜉 ) 𝑹𝑏
𝑇𝑸𝝈𝑑𝐴.
In the implementation these integrals are evaluated using 4-point Gaussian quadrature, 
where the integration point locations are given by 
𝜉∗ =
⎢⎡−
⎣
√3
,
√3
,
√3
, −
⎥⎤,
√3⎦
𝜂∗ =
⎢⎡−
⎣
√3
, −
√3
,
√3
,
⎥⎤.
√3⎦
Thus an integral is evaluated as 
∫ 𝜙(𝜉 , 𝜂)𝛔𝑑𝐴
≈ ∑ 𝜙(𝜉𝑖, 𝜂𝑖)𝛔𝑖𝐴𝑖
,
𝑖=1
(5.27)
(5.28)
LS-DYNA Theory Manual 
Cohesive Elements 
where 𝜙 is an arbitrary function of the iso-parametric coordinates, 𝐴𝑖 in the right hand 
side stands for the area of the cohesive layer and 𝛔𝑖 is the cohesive interface stress, both 
evaluated at and with respect to integration point i. 
5.4  Drilling constraint in shell ±29 
From  (5.8)  and  the  picture  of  shell  type  ±29  in  Figure  5.1,  we  see  that  rotational 
velocities  with  respect  to  the  adjacent  shell  normals  will  not  induce  translational 
velocities in the integration points, so a stabilization scheme is applied.  To this end we 
𝑚,  𝑖 = 1,2, 𝑗 = 3,4,  distances  that  are 
introduce  the  generalized  drilling  strains  δ𝑖
incremented by their respective  velocities 
𝑛  and  δ𝑗
𝑛 = 𝒏𝑡
𝛿 ̇
𝑚 = 𝒏𝑏
𝛿 ̇
𝑇{𝝎𝑖
𝑇{𝝎𝑗
𝑛𝑑21 − 𝑹21(𝒙̇2
𝑚𝑑34 − 𝑹34(𝒙̇3
𝑛 − 𝒙̇1
𝑚 − 𝒙̇4
𝑛)}, 𝑖 = 1,2,  
𝑚)}, 𝑗 = 3,4, 
where 
𝑑21 = ∣𝒙2
𝑑34 = ∣𝒙3
𝑛∣,
𝑛 − 𝒙1
𝑚∣, 
𝑚 − 𝒙4
and we make use of the following definitions for arbitrary vector 𝐯, 
𝑹21𝒗 =
𝑹34𝒗 =
𝑑21
𝑑34
(𝒙2
𝑛 − 𝒙1
𝑛) × 𝒗,
(𝒙3
𝑚 − 𝒙4
𝑚) × 𝒗.
(5.29)
(5.30)
(5.31)
A  characteristic  material  stiffness  𝐸,  typically  a  fraction  of  the  elastic  stiffness  of  the 
underlying cohesive material, is used to set up the drilling stress 
𝑛,
𝑛 = 𝐸𝛿𝑖
𝜍𝑖
𝑚,
𝑚 = 𝐸𝛿𝑗
𝜍𝑗
𝑖 = 1,2,
𝑗 = 3,4, 
(5.32)
and the stabilization nodal forces are evaluated as
Cohesive Elements 
LS-DYNA Theory Manual 
𝑇 𝐧𝑡, 𝐫1
𝑛 = 𝐴𝜍2
𝑚 = 𝐴𝜍3
𝑇 𝐧𝑏, 𝐫4
and these forces and moments are added to the structural ones in the previous section. 
𝑛+𝜍2
𝑛 = 𝐴(𝜍1
𝐟1
𝑛 = −𝐟1
𝐟2
𝑚 = −𝐟4
𝐟3
𝑚+𝜍4
𝑛 = 𝐴𝜍1
𝑛𝑑21𝐧𝑡, 
𝑚𝑑34𝐧𝑏, 
𝑚 = 𝐴𝜍4
𝑛)𝐑21
𝑛, 𝐫2
𝑚, 𝐫3
𝑚)𝐑34
𝑚 = 𝐴(𝜍3
𝐟4
𝑚𝑑34𝐧𝑏,
𝑛𝑑21𝐧𝑡,
(5.33)
5.5  Rotational masses in shell ±29 
The  rotational  mass  in  shell  ±29  is  determined  from  a  simple  energy  criterion.  
Assuming that the cohesive layer is thin and the layer spins with a rotational velocity 𝜔 
around axis 𝒒2, the kinetic energy from the nodal rotational masses 𝑚𝑟 is 
𝑊 =
(𝑚𝑟 + 𝑚𝑟 + 𝑚𝑟 + 𝑚𝑟)𝜔2 = 2𝑚𝑟𝜔2.
(5.34)
This  is  compared  to  the  corresponding  kinetic  energy  for  an  equivalent  solid  type  19 
cohesive layer, using that the shell type ±29 translational nodal mass 𝑚𝑡 is twice that of 
the solid type 19 nodal masses, 
𝑊 =
𝑚𝑡
(
+
𝑚𝑡
+
𝑚𝑡
+
𝑚𝑡
+
𝑚𝑡
+
𝑚𝑡
+
𝑚𝑡
+
𝑚𝑡
) (
𝜔)
=
𝑚𝑡𝑡2𝜔2, 
which results in 
𝑚𝑟 =
𝑚𝑡𝑡2.
(5.35)
(5.36)
5.6  Stiffness matrix in shell ±29 
The stiffness matrix is the sum of contributions from the constitutive law and the 
drilling force, and is for simplicity implemented for a force free configuration, i.e., 
𝝈 = 𝟎,
𝝇 = 𝟎,
(5.37)
where we have used the notation
LS-DYNA Theory Manual 
Cohesive Elements 
𝝇 =
𝜍1
⎤
⎡
𝜍2
⎥
⎢
. 
⎥
⎢
𝜍3
⎥
⎢
𝑚⎦
𝜍4
⎣
(5.38)
For a given integration point and referring to Equation (5.26) and (5.33), we collect these 
nodal force triplets into complete nodal vectors 𝒇  and 𝒈, associated with the constitutive 
and drilling part, respectively.  That is, 
𝒇 =
𝒇1
⎤
⎡
𝒓1
⎥
⎢
⎥
⎢
𝒇2
⎥
⎢
⎥
⎢
𝒓2
⎥
⎢
, 
⎥
⎢
𝒇3
⎥
⎢
⎥
⎢
𝒓3
⎥
⎢
𝒇4
⎥
⎢
𝑚⎦
𝒓4
⎣
(5.39)
and  the  same  expression  holds  for  𝒈.  Likewise  we  let  𝒗  be  the  collection  of  nodal 
velocities, i.e., 
𝒗 =
𝒙̇1
⎤
⎡
𝝎1
⎥
⎢
⎥
⎢
𝒙̇2
⎥
⎢
𝝎2
⎥
⎢
⎥
⎢
𝒙̇3
⎥
⎢
⎥
⎢
𝝎3
⎥
⎢
𝒙̇4
⎥
⎢
𝑚⎦
𝝎4
⎣
, 
(5.40)
and  note  that  we  can  identify  generalized  strain-displacement  matrices  𝑩𝑓   (3  by  24 
matrix) and 𝑩𝑔 (4 by 24 matrix) from (5.6) and (5.8) as well as (5.29) so that 
𝒅 ̇= 𝑩𝑓 𝒗,
𝜹 ̇ = 𝑩𝑔𝒗,
where we have collected the drilling kinematic velocities in a vector 
𝜹 ̇ =
𝛿 ̇
⎤
⎡
𝛿 ̇
⎥
⎢
⎥
⎢
⎥
⎢
𝛿 ̇
⎥
⎢
𝑚⎦
𝛿 ̇
⎣
With this notation we can rewrite (5.26) and (5.33) into a more compact form 
(5.41)
(5.42)
Cohesive Elements 
LS-DYNA Theory Manual 
𝒇 = 𝑩𝑓
𝑇𝝈𝐴,
𝒈 = 𝑩𝑔
𝑇𝝇𝐴,
(5.43)
with  𝐴  here  being  the  area  of  the  integration  point  of  interest.    The  stiffness  matrix  is 
then  simply  the  differentiation  of  these  force  vectors  with  respect  to  the  nodal 
coordinates, and by using (5.32), (5.37) and the chain rule of differentiation we get 
𝑲𝑓 = 𝑩𝑓
𝑩𝑓 𝐴,
𝑇 𝜕𝝈
𝜕𝒅
𝑇𝑩𝑔𝐴,
𝑲𝑔 = 𝐸𝑩𝑔
(5.44)
where 𝜕𝝈/𝜕𝒅 is the constitutive tangent from the cohesive material used.
LS-DYNA Theory Manual 
Belytschko Beam 
6  
Belytschko Beam 
The  Belytschko  beam  element  formulation  [Belytschko  et  al.    1977]  is  part  of  a 
family of structural finite elements, by Belytschko and other researchers that employ a 
‘co-rotational  technique’  in  the  element  formulation  for  treating  large  rotation.    This 
section  discusses  the  co-rotational  formulation,  since  the  formulation  is  most  easily 
described for a beam element, and then describes the beam theory used to formulate the 
co-rotational beam element. 
6.1  Co-rotational Technique 
from 
In  any  large  displacement  formulation,  the  goal  is  to  separate  the  deformation 
displacements 
the  deformation 
displacements give rise to strains and the associated generation of strain energy.  This 
separation  is  usually  accomplished  by  comparing  the  current  configuration  with  a 
reference configuration. 
the  rigid  body  displacements,  as  only 
The current configuration is a complete description of the deformed body in its 
current  spatial  location  and  orientation,  giving  locations  of  all  points  (nodes) 
comprising the body.  The reference configuration can be either the initial configuration 
of the body, i.e., nodal locations at time zero, or the configuration of the body at some 
other  state  (time).    Often  the  reference  configuration  is  chosen  to  be  the  previous 
configuration, say at time 𝑡𝑛 = 𝑡𝑛+1 − Δ𝑡. 
The  choice  of  the  reference  configuration  determines  the  type  of  deformations 
that  will  be  computed:    total  deformations  result  from  comparing  the  current 
configuration with the initial configuration, while incremental deformations result from 
comparing  with  the  previous  configuration.    In  most  time  stepping  (numerical) 
Lagrangian  formulations,  incremental  deformations  are  used  because  they  result  in 
significant simplifications of other algorithms, chiefly constitutive models.
Belytschko Beam 
LS-DYNA Theory Manual 
b2
¯Y
b1
^
e0
e0
X¯
(a)  Initial Configuration
^
Figure 6.1.  Co-rotational coordinate system:  (a) initial configuration, (b) rigid
rotational configuration and (c) deformed configuration. 
A direct comparison of the current configuration with the reference configuration 
does not result in a determination of the deformation, but rather provides the total (or 
incremental)  displacements.    We  will  use  the  unqualified  term  displacements  to  mean 
either  the  total  displacements  or  the  incremental  displacements,  depending  on  the 
choice of the reference configuration as the initial or the last state.  This is perhaps most 
obvious if the reference configuration is the initial configuration.  The direct comparison 
of  the  current  configuration  with  the  reference  configuration  yields  displacements, 
which  contain  components  due  to  deformations  and  rigid  body  motions.    The  task 
remains of separating the deformation and rigid body displacements.  The deformations 
are usually found by subtracting from the displacements an estimate of the rigid body 
displacements.  Exact rigid body displacements are usually only known for trivial cases 
where  they  are  prescribed  a  priori  as  part  of  a  displacement  field.    The  co-rotational 
formulations provide one such estimate of the rigid body displacements. 
The co-rotational formulation uses two types of coordinate systems:  one system 
associated with each element, i.e., element coordinates which deform with the element, 
and another associated with each node, i.e., body coordinates embedded in the nodes.  
(The term ‘body’ is used to avoid possible confusion from referring to these coordinates 
as ‘nodal’ coordinates.  Also, in the more general formulation presented in [Belytschko 
et al., 1977], the nodes could optionally be attached to rigid bodies.  Thus the term ‘body 
coordinates’  refers  to  a  system  of  coordinates  in  a  rigid  body,  of  which  a  node  is  a 
special case.)  These two coordinate systems are shown in the upper portion of Figure 
6.1. 
The element coordinate system is defined to have the local x-axis 𝐱̂ originating at 
node 𝐼 and terminating at node 𝐽; the local y-axis 𝐲̂ and, in three dimension, the local z-
axis  𝐳̂,  are  constructed  normal  to  𝐱̂.    The  element  coordinate  system  (𝐱̂, 𝐲̂, 𝐳̂)  and 
associated  unit  vector  triad  (𝐞1, 𝐞2, 𝐞3)  are  updated  at  every  time  step  by  the  same 
technique used to construct the initial system; thus the unit vector e1 deforms with the 
element since it always points from node 𝐼 to node 𝐽.
LS-DYNA Theory Manual 
Belytschko Beam 
^
^
e2
¯Y
b2
e1
b1
X¯
(b) Rigid Rotation Configuration
Figure 6.2.  Co-rotational coordinate system: (a) initial configuration, (b) rigid
rotational configuration and (c) deformed configuration. 
The  embedded  body  coordinate  system  is  initially  oriented  along  the  principal 
inertial axes; either the assembled nodal mass or associated rigid body inertial tensor is 
used  in  determining  the  inertial  principal  values  and  directions.    Although  the  initial 
orientation  of  the  body  axes  is  arbitrary,  the  selection  of  a  principal  inertia  coordinate 
system simplifies the rotational equations of motion, i.e., no inertial cross product terms 
are  present  in  the  rotational  equations  of  motion.    Because  the  body  coordinates  are 
fixed  in  the  node,  or  rigid  body,  they  rotate  and  translate  with  the  node  and  are 
updated  by  integrating  the  rotational  equations  of  motion,  as  will  be  described 
subsequently. 
The unit vectors of the two coordinate systems define rotational transformations 
between  the  global  coordinate  system  and  each  respective  coordinate  system.    These 
transformations  operate  on  vectors  with  global  components  𝐀 = (𝐴𝑥, 𝐴𝑦, 𝐴𝑧),  body 
coordinates  components  𝐀̅̅̅̅̅̅ = (𝐴̅𝑥, 𝐴̅𝑦, 𝐴̅𝑧),  and  element  coordinate  components  Â =
(𝐴̂𝑥, 𝐴̂𝑦, 𝐴̂𝑧) which are defined as: 
𝐀 =
{⎧𝐴𝑥
}⎫
𝐴𝑦
𝐴𝑧⎭}⎬
⎩{⎨
=
𝑏1𝑥
⎡
𝑏1𝑦
⎢⎢
𝑏1𝑧
⎣
𝑏2𝑥
𝑏2𝑦
𝑏2𝑧
𝑏3𝑥
⎤
𝑏3𝑦
⎥⎥
𝑏3𝑧⎦
{{⎧𝐴̅𝑥
}}⎫
𝐴̅𝑦
}}⎬
{{⎨
𝐴̅𝑧⎭
⎩
= [𝛌]{𝐀̅̅̅̅̅̅}, 
(6.1)
where  𝑏𝑖𝑥,  𝑏𝑖𝑦,  𝑏𝑖𝑧  are  the  global  components  of  the  body  coordinate  unit  vectors.  
Similarly for the element coordinate system: 
𝐀 =
{⎧𝐴𝑥
}⎫
𝐴𝑦
𝐴𝑧⎭}⎬
⎩{⎨
=
𝑒1𝑥
⎢⎡
𝑒1𝑦
𝑒1𝑧
⎣
𝑒2𝑥
𝑒2𝑦
𝑒2𝑧
𝑒3𝑥
⎥⎤
𝑒3𝑦
𝑒3𝑧⎦
⎧𝐴̂𝑥
⎫
}}
{{
𝐴̂𝑦
⎬
⎨
}}
{{
𝐴̂𝑧⎭
⎩
= [𝛍]{𝐀̂}, 
(6.2)
where 𝑒𝑖𝑥, 𝑒𝑖𝑦, 𝑒𝑖𝑧 are the global components of the element coordinate unit vectors.  The 
inverse transformations are defined by the matrix transpose, i.e., 
{𝐀̅̅̅̅̅̅} = [𝛌]T{𝐀}
{𝐀̂} = [𝛍]T{𝐀},
(6.3)
Belytschko Beam 
LS-DYNA Theory Manual 
¯Y
b2
^
e2
e1
b1
e0
X¯
(c) Deformed Configuration
^
Figure 6.3.  Co-rotational coordinate system:  (a) initial configuration, (b) rigid
rotational configuration and (c) deformed configuration. 
since these are proper rotational transformations. 
The  following  two  examples  illustrate  how  the  element  and  body  coordinate 
system  are  used  to  separate  the  deformations  and  rigid  body  displacements  from  the 
displacements: 
Rigid Rotation.  First, consider a rigid body rotation of the beam element about node 𝐼, 
as  shown  in  the  center  of  Figure  6.2,  i.e.,  consider  node  𝐼  to  be  a  pinned  connection.  
Because the beam does not deform during the rigid rotation, the orientation of the unit 
vector  𝐞1  in  the  initial  and  rotated  configuration  will  be  the  same  with  respect  to  the 
body coordinates.  If the body coordinate components of the initial element unit vector 
0  were  stored,  they  would  be  identical  to  the  body  coordinate  components  of  the 
𝐞1
current element unit vector e1. 
Deformation Rotation.  Next, consider node 𝐼 to be constrained against rotation, i.e., a 
clamped connection.  Now node 𝐽 is moved, as shown in the lower portion of Figure 6.3, 
causing the beam element to deform.  The updated element unit vector e1 is constructed 
and its body coordinate components are compared to the body coordinate components 
0.    Because  the  body  coordinate  system  did  not 
of  the  original  element  unit  vector  𝐞1
rotate,  as  node  I  was  constrained,  the  original  element  unit  vector  and  the  current 
element unit vector are not colinear.  Indeed, the angle between these two unit vectors is 
the amount of rotational deformation at node I, i.e., 
𝐞1 × 𝐞1
0 = 𝜃ℓ𝐞3.
(6.4)
Thus  the  co-rotational  formulation  separates  the  deformation  and  rigid  body 
deformations by using: 
•  a coordinate system that deforms with the element, i.e., the element coordinates; 
•  or  a  coordinate  system  that  rigidly  rotates  with  the  nodes,  i.e.,  the  body 
coordinates;
LS-DYNA Theory Manual 
Belytschko Beam 
Then  it  compares  the  current  orientation  of  the  element  coordinate  system  with  the 
initial element coordinate system, using the rigidly rotated body coordinate system, to 
determine the deformations.  
6.2  Belytschko Beam Element Formulation 
The  deformation  displacements  used 
in 
the  Belytschko  beam  element 
formulation are: 
where, 
𝐝̂T = {𝛿𝐼𝐽, 𝜃̂
𝑥𝐽𝐼, 𝜃̂
𝑦𝐼, 𝜃̂
𝑦𝐽, 𝜃̂
𝑧𝐼, 𝜃̂
𝑧𝐽},
(6.5)
𝛿𝐼𝐽 = length change 
𝜃̂
𝑥𝐽𝐼 = torsional deformation 
𝑧𝐼, 𝜃̂
𝑧𝐽 = bending rotation deformations 
𝑦𝐼, 𝜃̂
𝜃̂
𝑦𝐽, 𝜃̂
The  superscript  ^  emphasizes  that  these  quantities  are  defined  in  the  local  element 
coordinate system, and 𝐼 and 𝐽 are the nodes at the ends of the beam. 
The  beam  deformations,  defined  above  in  Equation  (6.5),  are  the  usual  small 
displacement beam deformations (see, for example, [Przemieniecki 1986]).  Indeed, one 
advantage  of  the  co-rotational  formulation  is  the  ease  with  which  existing  small 
displacement element formulations can be adapted to a large displacement formulation 
having  small  deformations  in  the  element  system.    Small  deformation  theories  can  be 
easily  accommodated  because  the  definition  of  the  local  element  coordinate  system  is 
independent  of  rigid  body  rotations  and  hence  deformation  displacement  can  be 
defined directly. 
6.2.1  Calculation of Deformations 
The  elongation  of  the  beam  is  calculated  directly  from  the  original  nodal 
coordinates (𝑋𝐼, 𝑌𝐼, 𝑍𝐼) and the total displacements (𝑢𝑥𝐼, 𝑢𝑦𝐼, 𝑢𝑧𝐼): 
𝛿𝐼𝐽 =
where 
𝑙 + 𝑙𝑜 [2(𝑋𝐽𝐼𝑢𝑥𝐽𝐼 + 𝑌𝐽𝐼𝑢𝑦𝐽𝐼 + 𝑍𝐽𝐼𝑢𝑧𝐽𝐼) + 𝑢𝑥𝐽𝐼
2 + 𝑢𝑦𝐽𝐼
2 + 𝑢𝑧𝐽𝐼
2 ], 
𝑋𝐽𝐼 = 𝑋𝐽 − 𝑋𝐼
𝑢𝑥𝐽𝐼 = 𝑢𝑥𝐽 − 𝑢𝑥𝐼, etc.
(6.6)
(6.7)
The deformation rotations are calculated using the body coordinate components 
0, as outlined in 
of the original element coordinate unit vector along the beam axis, i.e., 𝐞1
0 
the previous section.  Because the body coordinate components of initial unit vector 𝐞1
rotate  with  the  node,  in  the  deformed  configuration  it  indicates  the  direction  of  the
Belytschko Beam 
LS-DYNA Theory Manual 
0 
beam’s axis if no deformations had occurred.  Thus comparing the initial unit vector 𝐞1
with  its  current  orientation  𝐞1  indicates  the  magnitude  of  deformation  rotations.  
Forming the vector cross product between 𝐞1
0 and 𝐞1: 
𝐞1 × 𝐞1
0 = 𝜃̂
𝑦𝐞2 + 𝜃̂
𝑧𝐞3,
(6.8)
where 
𝜃̂
𝑦 = is the incremental deformation about the local 𝑦̂ axis 
𝜃̂
𝑧 = is the incremental deformation about the local 𝑧̂ axis 
The calculation is most conveniently performed by transforming the body components 
of the initial element vector into the current element coordinate system: 
⎫
⎧𝑒 ̂1𝑥
}}
{{
 0
𝑒 ̂1𝑦
⎬
⎨
}}
{{
0 ⎭
𝑒 ̂1𝑧
⎩
= [𝛍]T[𝛌]
⎫
⎧𝑒 ̅1𝑥
}}
{{
 0
𝑒 ̅1𝑦
⎬
⎨
}}
{{
0 ⎭
𝑒 ̅1𝑧
⎩
. 
Substituting the above into Equation (4.10) 
𝐞1 × 𝐞1
0 = det
𝐞1
 0
𝑒 ̂1𝑥
⎡
⎢
⎣
𝐞2
 0
𝑒 ̂1𝑦
𝐞3
 0
𝑒 ̂1𝑧
Thus, 
⎤ = −𝑒 ̂1𝑧
⎥
⎦
 0 𝐞2 + 𝑒 ̂1𝑦
 0 𝐞3 = 𝜃̂
𝑦𝐞2 + 𝜃̂
𝑧𝐞3. 
𝜃̂
𝑦 = −𝑒 ̂1𝑧
 0 .
𝜃̂
𝑧 = 𝑒 ̂1𝑦
(6.9)
(6.10)
(6.11)
The torsional deformation rotation is calculated from the vector cross product of 
initial  unit  vectors,  from  each  node  of  the  beam,  that  were  normal  to  the  axis  of  the 
 0   could  also  be  used.    The  result  from  this 
 0   and  𝑒 ̂3𝐽
beam,  i.e.,  𝑒 ̂2𝐼
vector cross product is then projected onto the current axis of the beam, i.e.,  
 0 ;  note  that  𝑒 ̂3𝐼
 0   and  𝑒 ̂2𝐽
𝜃̂
𝑥𝐽𝐼 = 𝐞1 ⋅ (𝐞̂2𝐼
0 × 𝐞̂2𝐽
0 ) = 𝐞1 ⋅ det
𝐞2
 0
𝑒 ̂𝑦2𝐼
 0
𝑒 ̂𝑦2𝐽
𝐞1
⎡
 0
𝑒 ̂𝑥2𝐼
⎢⎢
 0
𝑒 ̂𝑥2𝐽
⎣
 0  and 𝑒 ̅2𝐽
𝐞3
 0
𝑒 ̂𝑧2𝐼
 0
𝑒 ̂𝑧2𝐽
⎤
⎥⎥
⎦
= 𝑒 ̂𝑦2𝐼
 0 𝑒 ̂𝑧2𝐽
 0 − 𝑒 ̂𝑦2𝐽
 0 . 
 0 𝑒 ̂𝑧2𝐼
(6.12)
Note that the body components of 𝑒 ̅2𝐼
coordinate system before performing the indicated vector products. 
 0  are transformed into the current element 
6.2.2  Calculation of Internal Forces 
There are two methods for computing the internal forces for the Belytschko beam 
element formulation: 
1. 
2. 
functional  forms  relating  the  overall  response  of  the  beam,  e.g.,    moment-
curvature relations, 
direct through-the-thickness integration of the stress.
{⎧𝜃̂
}⎫
𝑦𝐼
𝑦𝐽⎭}⎬
⎩{⎨
𝜃̂
𝜃̂
𝑧𝐼
𝜃̂
𝑧𝐽
LS-DYNA Theory Manual 
Belytschko Beam 
Currently  only  the  former  method,  as  explained  subsequently,  is  implemented;  the 
direct integration method is detailed in [Belytschko et al., 1977]. 
Axial Force.  The internal axial force is calculated from the elongation of the beam 𝛿, as 
given by Equation (6.6), and an axial stiffness: 
𝑓 ̂
𝑥𝐽 = 𝐾𝑎𝛿,
(6.13)
where 
𝐾𝑎 =
𝐴𝐸
𝑙0 = is the axial stiffness 
𝐴 = cross sectional area of the beam 
𝐸 = Young's Modulus 
𝑙0 = original length of the beam 
Bending Moments.  The bending moments are related to the deformation rotations by 
{
𝑚̂𝑦𝐼
𝑚̂𝑦𝐽
} =
𝐾𝑦
1 + 𝜙𝑦
4 + 𝜙𝑦2 − 𝜙𝑦
[
2 − 𝜙𝑦4 + 𝜙𝑦
]
, 
(6.14a)
4 + 𝜙𝑧2 − 𝜙𝑧
2 − 𝜙𝑧4 + 𝜙𝑧
where  Equation  (6.14a)  is  for  bending  in  the  𝐱̂ − 𝐳̂  plane  and  Equation  (6.14b)  is  for 
bending in the 𝐱̂ − 𝐲̂ plane.  The bending constants are given by 
𝑚̂𝑧𝐼
{
𝑚̂𝑧𝐽
(6.14b)
} =
] {
}, 
[
𝐾𝑧
1 + 𝜙𝑧
𝑏 =
𝐾𝑦
𝑏 =
𝐾𝑧
𝐸𝐼𝑦𝑦
𝑙0  
𝐸𝐼𝑧𝑧
𝑙0
𝐼𝑦𝑦 = ∫ ∫ 𝑧̂2𝑑𝑦̂𝑑𝑧̂ 
𝐼𝑧𝑧 = ∫ ∫ 𝑦̂2𝑑𝑦̂𝑑𝑧̂ 
𝜙𝑦 =
𝜙𝑧 =
12𝐸𝐼𝑦𝑦
𝐺𝐴𝑠𝑙2  
12𝐸𝐼𝑧𝑧
𝐺𝐴𝑠𝑙2 . 
(6.15a)
(6.15b)
(6.15c)
(6.15d)
(6.15e)
(6.15f)
Hence 𝜙 is the shear factor, 𝐺 the shear modulus, and 𝐴𝑠 is the effective area in shear. 
Torsional Moment.  The torsional moment is calculated from the torsional deformation 
rotation as
Belytschko Beam 
LS-DYNA Theory Manual 
where 
and, 
𝑚̂𝑥𝐽 = 𝐾𝑡𝜃̂
𝑥𝐽𝐼,
𝐾𝑡 =
𝐺𝐽
𝑙0 ,
𝐽 = ∫ ∫ 𝑦̂𝑧̂𝑑𝑦̂𝑑𝑧̂. 
(6.16)
(6.17)
(6.18)
The  above  forces  are  conjugate  to  the  deformation  displacements  given 
previously in Equation (6.5), i.e., 
𝐝̂T = {𝛿𝐼𝐽, 𝜃̂
𝑥𝐽𝐼, 𝜃̂
𝑦𝐼, 𝜃̂
𝑦𝐽, 𝜃̂
𝑧𝐼, 𝜃̂
𝑧𝐽},
where 
And with 
𝐝̂T𝐟 ̂ = 𝑊int.
𝐟 ̂ T = {𝑓 ̂
𝑥𝐽, 𝑚̂𝑥𝐽, 𝑚̂𝑦𝐼, 𝑚̂𝑦𝐽, 𝑚̂𝑧𝐼, 𝑚̂𝑧𝐽}.
The remaining internal force components are found from equilibrium: 
𝑓 ̂
𝑧𝐼 = −
𝑥𝐼 = −𝑓 ̂
𝑓 ̂
𝑥𝐽
𝑚̂𝑦𝐼 + 𝑚̂𝑦𝐽
𝑙0
𝑚̂𝑧𝐼 + 𝑚̂𝑧𝐽
𝑙0
𝑓 ̂
𝑦𝐽 = −
𝑚̂𝑥𝐼 = −𝑚̂𝑥𝐽
𝑧𝐼 = −𝑓 ̂
𝑓 ̂
𝑧𝐽
𝑦𝐼 = −𝑓 ̂
𝑓 ̂
𝑦𝐽
(6.19)
(6.20)
(6.21)
(6.22)
6.2.3  Updating the Body Coordinate Unit Vectors 
The  body  coordinate  unit  vectors  are  updated  using  the  Newmark  𝛽-Method 
[Newmark 1959] with 𝛽 = 0, which is almost identical to the central difference method 
[Belytschko  1974].    In  particular,  the  body  component  unit  vectors  are  updated  using 
the formula 
 𝑗+1 = 𝐛𝑖
𝐛𝑖
 𝑗 + Δ𝑡
d𝐛𝑖
d𝑡
Δ𝑡2
d2𝐛𝑖
d𝑡2 ,
+
(6.23)
where  the  superscripts  refer  to  the  time  step  and  the  subscripts  refer  to  the  three  unit 
vectors  comprising  the  body  coordinate  triad.    The  time  derivatives  in  the  above 
equation are replaced by their equivalent forms from vector analysis: 
= 𝛚 × 𝐛𝑖 
 𝑗
d𝐛𝑖
d𝑡
 𝑗
d2𝐛𝑖
d𝑡2 = 𝛚 × (𝛚 × 𝐛𝑖) + (𝛂𝑖 × 𝐛𝑖),
(6.24)
LS-DYNA Theory Manual 
Belytschko Beam 
where 𝜔  and 𝛼  are  vectors  of  angular velocity and  acceleration,  respectively, obtained 
from  the  rotational  equations  of  motion.    With  the  above  relations  substituted  into 
Equation (6.23), the update formula for the unit vectors becomes 
 𝑗+1 = 𝐛𝑖
𝐛𝑖
 𝑗 + Δ𝑡(𝛚 × 𝐛𝑖) +
Δ𝑡2
{[𝛚 × (𝛚 × 𝐛𝑖) + (𝛂𝑖 × 𝐛𝑖)]}. 
(6.25)
To  obtain  the  formulation  for  the  updated  components  of  the  unit  vectors,  the 
body coordinate system is temporarily considered to be fixed and then the dot product 
of Equation (6.25) is formed with the unit vector to be updated.  For example, to update 
the 𝑥̅ component of 𝐛3, the dot product of Equation (6.25), with 𝑖 = 3, is formed with b1, 
which can be simplified to the relation 
 𝑗+1 = 𝐛1
𝑏̅
𝑥3
 𝑗 ⋅ 𝐛3
 𝑗+1 = Δ𝑡𝜔𝑦
 𝑗 +
Similarly, 
 𝑗+1 = 𝐛2
𝑏̅
𝑦3
 𝑗 ⋅ 𝐛3
 𝑗+1 = Δ𝑡𝜔𝑥
 𝑗 +
 𝑗+1 = 𝐛1
𝑏̅
𝑧3
 𝑗 ⋅ 𝐛2
 𝑗+1 = Δ𝑡𝜔𝑧
𝑗 +
Δ𝑡2
Δ𝑡2
Δ𝑡2
(𝜔𝑥
 𝑗𝜔𝑧
 𝑗 + 𝛼𝑦
 𝑗),
(𝜔𝑦
 𝑗𝜔𝑧
 𝑗 + 𝛼𝑥
 𝑗) 
(6.26)
(6.27)
(𝜔𝑥
 𝑗𝜔𝑦
 𝑗 + 𝛼𝑧
 𝑗).
 𝑗+1  are  found  by  using  normality  and 
The  remaining  components  𝐛3
orthogonality, where it is assumed that the angular velocities w are small during a time 
 𝑗+1 is a 
step so that the quadratic terms in the update relations can be ignored.  Since 𝐛3
unit vector, normality provides the relation 
 𝑗+1  and  𝐛1
 𝑗+1 = √1 − (𝑏̅
𝑏̅
𝑧3
 𝑗+1)
𝑥3
− (𝑏̅
 𝑗+1)
𝑦3
.
Next, if it is assumed that 𝑏̅
 𝑗+1 ≈ 1, orthogonality yields 
𝑥1
 𝑗+1 = −
𝑏̅
𝑧1
𝑗+1 + 𝑏̅
𝑏̅
𝑥3
𝑗+1
𝑦3
. 
𝑗+1𝑏̅
𝑦1
 𝑗+1
𝑏̅
𝑧3
The component 𝑏̅
 𝑗+1 is then found by enforcing normality: 
𝑥1
 𝑗+1 = √1 − (𝑏̅
𝑏̅
𝑥1
 𝑗+1)
𝑦1
− (𝑏̅
 𝑗+1)
𝑧1
.
(6.28)
(6.29)
(6.30)
The  updated  components  of  𝐛1  and  𝐛3  are  defined  relative  to  the  body coordinates  at 
time  step  𝑗.    To  complete  the  update  and  define  the  transformation  matrix,  Equation 
(6.1), at time step 𝑗 + 1, the updated unit vectors 𝐛1 and 𝐛3 are transformed to the global 
coordinate system, using Equation (6.1) with [𝛌] defined at step 𝑗, and their vector cross 
product is used to form 𝐛2.
LS-DYNA Theory Manual 
Hughes-Liu Beam 
7    
Hughes-Liu Beam 
The Hughes-Liu beam element formulation, based on the shell [Hughes and Liu 
1981a,  1981b]  discussed  later,  was  the  first  beam  element  we  implemented.    It  has 
several desirable qualities: 
•  It  is  incrementally  objective  (rigid  body  rotations  do  not  generate  strains), 
allowing for the treatment of finite strains that occur in many practical applica-
tions; 
•  It  is  simple,  which  usually  translates  into  computational  efficiency  and  robust-
ness 
•  It  is  compatible  with  the  brick  elements,  because  the  element  is  based  on  a 
degenerated brick element formulation;  
•  It  includes  finite  transverse  shear  strains.    The  added  computations  needed  to 
retain  this  strain  component,  compare  to  those  for  the  assumption  of  no  trans-
verse shear strain, are insignificant. 
7.1  Geometry 
The Hughes-Liu beam element is based on a degeneration of the isoparametric 8-
node  solid  element,  an  approach  originated  by  Ahmad  et  al.,  [1970].    Recall  the  solid 
element isoparametric mapping of the biunit cube 
with, 
𝐱(𝜉 , 𝜂, 𝜁 ) = ∑ 𝑁𝑎(𝜉 , 𝜂, 𝜁 )𝑥𝑎
𝑎=1
,
𝑁𝑎(𝜉 , 𝜂, 𝜁 ) =
(1 + 𝜉𝑎𝜉 )(1 + 𝜂𝑎𝜂)(1 + 𝜁𝑎𝜁 )
,
(7.1)
(7.2)
Hughes-Liu Beam 
LS-DYNA Theory Manual 
where 𝐱 is an arbitrary point in the element, (𝜉 , 𝜂, 𝜁 ) are the parametric coordinates, 𝐱𝑎 
are  the  global  nodal  coordinates  of  node  𝑎,  and  𝑁𝑎  are  the  element  shape  functions 
evaluated at node 𝑎, i.e.,  (𝜉𝑎, 𝜂𝑎, 𝜁𝑎) are  (𝜉 , 𝜂, 𝜁 ) evaluated at node 𝑎. 
In the beam geometry, 𝜉  determines the location along the axis of the beam and 
the coordinate pair  (𝜂, 𝜁 ) defines a point on the cross section.  To degenerate the 8-node 
brick geometry into the 2-node beam geometry, the four nodes at 𝜉 = −1 and at 𝜉 = 1 
are combined into a single node with three translational and three rotational degrees of 
freedom.  Orthogonal, inextensible nodal fibers are defined at each node for treating the 
rotational degrees of freedom.  Figure 7.1 shows a schematic of the biunit cube and the 
beam element.  The mapping of the biunit cube into the beam element is separated into 
three parts: 
𝐱(𝜉 , 𝜂, 𝜁 ) = 𝐱̅(𝜉 ) + 𝐗(𝜉 , 𝜂, 𝜁 ),
= 𝐱̅(𝜉 ) + 𝐗𝜁 (𝜉 , 𝜁 ) + 𝐗𝜂(𝜉 , 𝜂),
(7.3)
where 𝐱̅ denotes a position vector to a point on the reference axis of the beam, and 𝐗𝜁  
 are position vectors at point 𝐱̅ on the axis that define the fiber directions through 
and 𝐗𝜂
Biunit Cube
Beam Element
+1
ζ¯
-1
Nodal fibers
Top Surface
z+
x+
x^
x¯
x^
x-
Bottom Surface
z-
Figure 7.1.  Hughes-Liu beam element.
LS-DYNA Theory Manual 
Hughes-Liu Beam 
that point.  In particular, 
,
𝐱̅(𝜉 ) = ∑ 𝑁𝑎(𝜉 )𝐱̅𝑎
𝑎=1
𝐗𝜂(𝜉 , 𝜂) = ∑ 𝑁𝑎(𝜉 )𝐗𝜂𝑎(𝜂)
𝑎=1
.
𝐗𝜁 (𝜉 , 𝜁 ) = ∑ 𝑁𝑎(𝜉 )𝐗𝜁𝑎(𝜁 )
𝑎=1
, 
(7.4)
With  this  description,  arbitrary  points  on  the  reference  line  𝐱̅  are  interpolated  by  the 
one- dimensional shape function 𝑁(𝜉 ) operating on the global position of the two beam 
nodes  that  define  the  reference  axis,  i.e.,  𝐱̅a.    Points  off  the  reference  axis  are  further 
interpolated by using a one-dimensional  shape function along the fiber directions, i.e., 
𝐗𝜂𝑎(𝜂) and 𝐗𝜁𝑎(𝜁 ) where 
𝐗𝜂𝑎(𝜂) = 𝑧𝜂𝑎(𝜂)𝐗̂𝜂𝑎 
𝑧𝜂𝑎(𝜂) = 𝑁+(𝜂)𝑧𝜂𝑎
𝐗𝜁𝑎(𝜁 ) = 𝑧𝜁𝑎(𝜁 )𝐗̂𝜁𝑎
𝑧𝜁𝑎(𝜁 ) = 𝑁+(𝜁 )𝑧𝜁𝑎
−  
+ + 𝑁−(𝜂)𝑧𝜂𝑎
+ + 𝑁−(𝜁 )𝑧𝜁𝑎
−  
𝑁+(𝜂) =
𝑁−(𝜂) =
(1 + 𝜂)
(1 − 𝜂)
𝑁+(𝜁 ) =
𝑁−(𝜁 ) =
(1 + 𝜁 )
(1 − 𝜁 )
(7.5)
where 𝑧𝜁 (𝜁 ) and 𝑧𝜂(𝜂) are “thickness functions”. 
The Hughes-Liu beam formulation uses four position vectors, in addition to 𝜉 , to 
locate  the  reference  axis  and  define  the  initial  fiber  directions.    Consider  the  two 
−   located  on  the  top  and  bottom  surfaces,  respectively,  at 
position  vectors  𝐱𝜁𝑎
node 𝑎.  Then 
+   and  𝐱𝜁𝑎
+ ,
− + (1 + 𝜁 ̅)𝐱𝜁𝑎
, 
𝐱̅𝜁𝑎 =
𝐗̂𝜁𝑎 =
(1 − 𝜁 ̅)𝐱𝜁𝑎
+ − 𝐱𝜁𝑎
− )
(𝐱𝜁𝑎
+ − 𝐱𝜁𝑎
− ∥
∥𝐱𝜁𝑎
(1 − 𝜁 ̅)∥𝐱𝜁𝑎
− = −
𝑧𝜁𝑎
+ =
𝑧𝜁𝑎
+ − 𝐱𝜁𝑎
− ∥, 
(1 + 𝜁 ̅)∥𝐱𝜁𝑎
+ − 𝐱𝜁𝑎
− ∥, 
+ ,
− + (1 + 𝜁 ̅)𝐱𝜂𝑎
𝐱̅𝜂𝑎 =
𝐗̂𝜂𝑎 =
(1 − 𝜁 ̅)𝐱𝜂𝑎
+ − 𝐱𝜂𝑎
− )
(𝐱𝜂𝑎
+ − 𝐱𝜂𝑎
− ∥
∥𝐱𝜂𝑎
− = −
𝑧𝜂𝑎
(1 − 𝜂̅)∥𝐱𝜂𝑎
+ =
𝑧𝜂𝑎
, 
+ − 𝐱𝜂𝑎
− ∥, 
(1 + 𝜂̅)∥𝐱𝜂𝑎
+ − 𝐱𝜂𝑎
− ∥, 
(7.6)
where  ‖ ⋅ ‖  is  the  Euclidean  norm.    The  reference  surface  may  be  located  at  the 
midsurface  of  the  beam  or  offset  at  the  outer  surfaces.    This  capability  is  useful  in 
several  practical  situations  involving  contact  surfaces,  connection  of  beam  elements  to 
solid  elements,  and  offsetting  elements  such  as  for  beam  stiffeners  in  stiffened  shells.  
The  reference  surfaces  are  located  within  the  beam  element  by  specifying  the  value  of 
the parameters 𝜂̅ and 𝜁 ̅, .  When these parameters take 
on the values –1 or +1, the reference axis is located on the outer surfaces of the beam.  If 
they are set to zero, the reference axis is at the center.
Hughes-Liu Beam 
LS-DYNA Theory Manual 
The  same  parametric  representation  used  to describe  the  geometry  of  the  beam 
elements  is  used  to  interpolate  the  beam  element  displacements,  i.e.,  an  isoparametric 
representation.    Again  the  displacements  are  separated  into  the  reference  axis 
displacements and rotations associated with the fiber directions: 
𝐮(𝜉 , 𝜂, 𝜁 ) = 𝐮̅̅̅̅(𝜉 ) + 𝐔(𝜉 , 𝜂, 𝜁 ),
= 𝐮̅̅̅̅(𝜉 ) + 𝐔𝜁 (𝜉 , 𝜁 ) + 𝐔𝜂(𝜉 , 𝜂).
The reference axis is interpolated as usual 
𝐮̅̅̅̅(𝜉 ) = ∑ 𝑁𝑎(𝜉 )𝐮̅̅̅̅𝑎
𝑎=1
. 
The displacements are also interpolated along the reference axis 
𝐔𝜂(𝜉 , 𝜂) = ∑ 𝑁𝑎(𝜉 )𝐔𝜂𝑎(𝜂),
𝑎=1
𝐔𝜁 (𝜉 , 𝜁 ) = ∑ 𝑁𝑎(𝜉 )𝐔𝜁𝑎(𝜁 )
𝑎=1
. 
The fiber displacement is interpolated consistently with the thickness, 
𝐔𝜂𝑎(𝜂) = 𝑧𝜂𝑎(𝜂)𝐔̂𝜂𝑎,
𝐔𝜁𝑎(𝜁 ) = 𝑧𝜁𝑎(𝜁 )𝐔̂𝜁𝑎, 
(7.7)
(7.8)
(7.9)
(7.10)
where 𝐮 is the displacement of a generic point, 𝐮̅̅̅̅ is the displacement of a point on the 
reference surface, and 𝑈 is the “fiber displacement” rotations.  The motion of the fibers 
can be interpreted as either displacements or rotations as will be discussed. 
Hughes  and  Liu  introduced  the  notation  that  follows,  and  the  associated 
schematic  shown  in  Figure  7.2,  to  describe  the  current  deformed  configuration  with 
respect to the reference configuration.   
𝐲 = 𝐲̅̅̅̅ + 𝐘, 
𝐲̅̅̅̅ = 𝐱̅ + 𝐮̅̅̅̅,
𝐲̅̅̅̅𝑎 = 𝐱̅𝑎 + 𝐮̅̅̅̅𝑎,
𝐘 = 𝐗 + 𝐔,
𝐘𝑎 = 𝐗𝑎 + 𝐔𝑎,
𝐘̂𝜂𝑎 = 𝐗̂𝜂𝑎 + 𝐔̂𝜂𝑎,
𝐘̂𝜁𝑎 = 𝐗̂𝜁𝑎 + 𝐔̂𝜁𝑎,
(7.11)
In  the  above  relations,  and  in  Figure  7.2,  the  𝐱  quantities  refer  to  the  reference 
configuration, the 𝐲 quantities refer to the updated (deformed) configuration and the 𝐮 
quantities are the displacements.  The notation consistently uses a superscript bar (⋅ ̅) to 
indicate  reference  surface  quantities,  a  superscript  caret  (⋅ ̂)  to  indicate  unit  vector 
quantities,  lower  case  letter  for  translational  displacements,  and  upper  case  letters  for 
fiber  displacements.    Thus  to  update  to  the  deformed  configuration,  two  vector 
quantities  are  needed:    the  reference  surface  displacement  𝐮̅̅̅̅  and  the  associated  nodal 
fiber displacement 𝐔.  The nodal fiber displacements are defined in the fiber coordinate 
system, described in the next subsection.
LS-DYNA Theory Manual 
Hughes-Liu Beam 
(parallel construction)
reference axis in
undeformed 
geometry
u¯
Deformed Configuration
Reference Surface
x¯
Figure 7.2.  Schematic of deformed configuration displacements and position
vectors. 
7.2  Fiber Coordinate System 
For  a  beam  element,  the  known  quantities  will  be  the  displacements  of  the 
reference  surface  𝑢̅  obtained  from  the  translational  equations  of  motion  and  the 
rotational  quantities  at  each  node  obtained  from  the  rotational  equations  of  motion.  
What remains to complete the kinematics is a relation between nodal rotations and fiber 
displacements 𝐔.  The linearized relationships between the incremental components Δ𝐔̂ 
the incremental rotations are given by  
⎧Δ𝑈̂𝜂1
⎫
}}
{{
Δ𝑈̂𝜂2
⎬
⎨
}}
{{
Δ𝑈̂𝜂3⎭
⎩
⎧Δ𝑈̂𝜁1
⎫
}}
{{
Δ𝑈̂𝜁2
⎬
⎨
}}
{{
Δ𝑈̂𝜁3⎭
⎩
=
=
⎡
⎢⎢⎢
−𝑌̂𝜂3
𝑌̂𝜂2 −𝑌̂𝜂1
⎣
⎡
⎢⎢⎢
−𝑌̂𝜁3
𝑌̂𝜁2 −𝑌̂𝜁1
⎣
𝑌̂𝜂3 −𝑌̂𝜂2
⎤
⎥⎥⎥
𝑌̂𝜂1
0 ⎦
𝑌̂𝜁3 −𝑌̂𝜁2
⎤
⎥⎥⎥
𝑌̂𝜁1
0 ⎦
{⎧Δ𝜃1
}⎫
Δ𝜃2
Δ𝜃3⎭}⎬
⎩{⎨
{⎧Δ𝜃1
}⎫
Δ𝜃2
Δ𝜃3⎭}⎬
⎩{⎨
= 𝐡𝜂Δ𝛉, 
= 𝐡𝜁 Δ𝛉. 
(7.12)
Equations (7.12) are used to transform the incremental fiber tip displacements to 
rotational increments in the equations of motion.  The second-order accurate rotational 
update  formulation  due  to  Hughes  and  Winget  [1980]  is  used  to  update  the  fiber 
vectors: 
then 
LS-DYNA Draft 
𝑌̂
𝑌̂
𝑛+1 = 𝑅𝑖𝑗(Δ𝜃)𝑌̂𝜂𝑖
𝑛,
𝜂𝑖
 𝑛+1 = 𝑅𝑖𝑗(Δ𝜃)𝑌̂
 𝑛,
𝜁𝑖
𝜁𝑖
Hughes-Liu Beam 
LS-DYNA Theory Manual 
Δ𝐔̂𝜂𝑎 = 𝐘̂𝜂𝑎
Δ𝐔̂𝜁𝑎 = 𝐘̂
𝑛+1 − 𝐘̂𝜂𝑎
𝑛 ,
𝑛+1 − 𝐘̂𝜁𝑎
𝑛 ,
𝜁𝑎
where 
𝑅𝑖𝑗(Δ𝜃) = 𝛿𝑖𝑗 +
(2𝛿𝑖𝑗 + Δ𝑆𝑖𝑘)Δ𝑆𝑖𝑘
2𝐷
Δ𝑆𝑖𝑗 = 𝑒𝑖𝑘𝑗Δ𝜃𝑘, 
, 
(7.14)
(7.15)
2𝐷 = 2 +
(Δ𝜃1
 2 + Δ𝜃2
 2 + Δ𝜃3
 2).
Here 𝛿𝑖𝑗 is the Kronecker delta and 𝑒𝑖𝑘𝑗 is the permutation tensor. 
7.2.1  Local Coordinate System 
In  addition  to  the  above  described  fiber  coordinate  system,  a  local  coordinate 
system  is  needed  to  enforce  the  zero  normal  stress  conditions  transverse  to  the  axis.  
The orthonormal basis with two directions 𝐞̂2 and 𝐞̂3 normal to the axis of the beam is 
constructed as follows: 
𝐞̂1 =
𝐞′2 =
,
𝐲̅̅̅̅2 − 𝐲̅̅̅̅1
∥𝐲̅̅̅̅2 − 𝐲̅̅̅̅1∥
𝐘̂𝜂1 + 𝐘̂𝜂2
∥𝐘̂𝜂1 + 𝐘̂𝜂2∥
. 
From the vector cross product of these local tangents. 
and to complete this orthonormal basis, the vector 
𝐞̂3 = 𝐞̂1 × 𝐞′2,
𝐞̂2 = 𝐞̂3 × 𝐞̂1,
(7.16)
(7.17)
(7.18)
is defined.  This coordinate system rigidly rotates with the deformations of the element. 
The transformation of vectors from the global to the local coordinate system can 
now be defined in terms of the basis vectors as 
𝐀̂ =
⎧𝐴̂𝑥
⎫
}}
{{
𝐴̂𝑦
⎬
⎨
}}
{{
𝐴̂𝑧⎭
⎩
=
𝑒1𝑥
⎢⎡
𝑒1𝑦
𝑒1𝑧
⎣
𝑒2𝑥
𝑒2𝑦
𝑒2𝑧
𝑒3𝑥
⎥⎤
𝑒3𝑦
𝑒3𝑧⎦
{⎧𝐴𝑥
}⎫
𝐴𝑦
𝐴𝑧⎭}⎬
⎩{⎨
= [𝐪]{𝐀}, 
(7.19)
where 𝑒𝑖𝑥, 𝑒𝑖𝑦, 𝑒𝑖𝑧 are the global components of the local coordinate unit vectors, 𝐀̂ is a 
vector in the local coordinates, and 𝐀 is the same vector in the global coordinate system.
LS-DYNA Theory Manual 
Hughes-Liu Beam 
7.3  Strains and Stress Update 
7.3.1  Incremental Strain and Spin Tensors 
The strain and spin increments are calculated from the incremental displacement 
gradient 
𝐺𝑖𝑗 =
∂Δ𝑢𝑖
∂𝑦𝑗
,
(7.20)
where Δ𝑢𝑖 are the incremental displacements and 𝑦𝑗 are the deformed coordinates.  The 
incremental strain and spin tensors are defined as the symmetric and skew-symmetric 
parts, respectively, of 𝐺𝑖𝑗: 
Δ𝜀𝑖𝑗 =
Δ𝜔𝑖𝑗 =
(𝐺𝑖𝑗 + 𝐺𝑗𝑖),
(𝐺𝑖𝑗 − 𝐺𝑗𝑖).
(7.21)
The  incremental  spin  tensor  Δ𝜔𝑖𝑗  is  used  as  an  approximation  to  the  rotational 
contribution  of  the  Jaumann  rate  of  the  stress  tensor;  in  an  implicit  implementation 
[Hallquist  1981b]  the  more  accurate  Hughes-Winget  [1980]  transformation  matrix  is 
used, Equation (7.15), with the incremental spin tensor for the rotational update.  Here 
the Jaumann rate update is approximated as 
𝜎 𝑖𝑗 = 𝜎𝑖𝑗
𝑛 + 𝜎𝑖𝑝
𝑛 Δ𝜔𝑝𝑗 + 𝜎𝑗𝑝
𝑛 Δ𝜔𝑝𝑖,
(7.22)
where  the  superscripts  on  the  stress  tensor  refer  to  the  updated  (𝑛 + 1)  and  reference 
(𝑛)  configurations.    This  update  of  the  stress  tensor  is  applied  before  the  constitutive 
evaluation, and the stress and strain are stored in the global coordinate system. 
7.3.2  Stress Update 
To  evaluate  the  constitutive  relation,  the  stresses  and  strain  increments  are 
rotated from the global to the local coordinate system using the transformation defined 
previously in Equation (7.19), viz. 
𝑙𝑛
𝜎𝑖𝑗
Δ𝜀𝑖𝑗
= 𝑞𝑖𝑘𝜎 𝑘𝑛𝑞𝑗𝑛,
 𝑙 = 𝑞𝑖𝑘Δ𝜀𝑘𝑛𝑞𝑗𝑛,
(7.23)
where the superscript 𝑙 indicates components in the local coordinate system.  The stress 
is updated incrementally: 
𝑙𝑛+1
𝜎𝑖𝑗
𝑙𝑛
= 𝜎𝑖𝑗
+ Δ𝜎𝑖𝑗
𝑛+1
2,
and rotated back to the global system: 
𝑙𝑛+1
𝑛+1 = 𝑞𝑘𝑖𝜎𝑘𝑛
𝜎𝑖𝑗
𝑞𝑛𝑗,
(7.24)
(7.25)
Hughes-Liu Beam 
LS-DYNA Theory Manual 
before computing the internal force vector. 
7.3.3  Incremental Strain-Displacement Relations 
After  the  constitutive  evaluation  is  completed,  the  fully  updated  stresses  are 
rotated  back  to  the  global  coordinate  system.    These  global  stresses  are  then  used  to 
update the internal force vector 
int = ∫ 𝐁𝑎
𝐟𝑎
T𝛔𝑑𝜐,
(7.26)
int are the internal forces at node 𝑎 and 𝐁𝑎 is the strain-displacement matrix in 
where 𝐟𝑎
the global coordinate system associated with the displacements at node 𝑎.  The 𝐁 matrix 
relates  six  global  strain  components  to  eighteen  incremental  displacements  [three 
translational displacements per node and the six incremental fiber tip displacements of 
Equation (7.14)].  It is convenient to partition the 𝐁 matrix: 
Each 𝐵𝑎 sub matrix is further partitioned into a portion due to strain and spin with the 
following sub matrix definitions: 
𝐁 = [𝐁1, 𝐁2].
(7.27)
𝐵1
⎡
𝐵2
⎢
⎢
⎢
⎢
𝐵2 𝐵1
⎢
⎢
𝐵3
⎣
𝐵3
𝐵3 𝐵2
𝐵4
𝐵5
𝐵5 𝐵4
𝐵1 𝐵6
𝐵6
𝐵6 𝐵5
𝐵7
𝐵8
𝐵8 𝐵7
𝐵4 𝐵9
⎤
⎥
⎥
𝐵9
⎥
, 
⎥
⎥
𝐵9 𝐵8
⎥
𝐵7⎦
𝐁𝑎 =
where, 
𝐵𝑖 =
⎧
{
{
{
{
{
⎨
{
{
{
{
{
⎩
𝑁𝑎,𝑖 =
(𝑁𝑎𝑧𝜂𝑎)
,𝑖−3
(𝑁𝑎𝑧𝜁𝑎)
,𝑖−6
=
=
𝜕𝑁𝑎
𝜕𝑦𝑖
𝜕(𝑁𝑎𝑧𝜂𝑎)
𝜕𝑦𝑖−3
𝜕(𝑁𝑎𝑧𝜁𝑎)
𝜕𝑦𝑖−6
𝑖 = 1,2,3
𝑖 = 4,5,6
. 
𝑖 = 7,8,9
(7.28)
(7.29)
With respect to the strain-displacement relations, note that: 
•  The  derivative  of  the  shape  functions  are  taken  with  respect  to  the  global 
coordinates; 
•  The  𝐁  matrix  is  computed  on  the  cross-section  located  at  the  mid-point  of  the 
axis; 
•  The resulting 𝐁 matrix is a 6 × 18 matrix.  
The internal force, 𝑓 , given by 
int
𝐟′ = 𝐓T𝐟𝑎
7-8 (Hughes-Liu Beam)
LS-DYNA Theory Manual 
Hughes-Liu Beam 
11
12
10
16
13
15
14
Figure  7.3.    Integration  possibilities  for  rectangular  cross  sections  in  the 
Hughes-Liu beam element. 
is assembled into the global right hand side internal force vector.  𝐓 is defined as (also 
see Equation (7.12): 
𝐓 =
⎤
⎡
𝟎 𝐡𝜂
, 
⎥
⎢
𝟎 𝐡𝜁 ⎦
⎣
(7.31)
where 𝐈 the 3 × 3 identity matrix. 
7.3.4  Spatial Integration 
The integration of Equation (7.26)  for the beam element is performed with one- 
point integration along the axis and multiple points in the cross section.  For rectangular 
cross sections, a variety of choices are available as is shown in Figure 7.3.  The beam has 
no zero energy or locking modes.
Hughes-Liu Beam 
LS-DYNA Theory Manual 
st
tt
Figure 7.4.  Specification of the nodal thickness, 𝑠𝑡 and 𝑡𝑡, for a beam with an
arbitrary cross-section. 
For  the  user  defined  rule,  it  is  necessary  to  specify  the  number  of  integration 
points and the relative area for the total cross section: 
𝐴𝑟 =
𝐬𝑡 ⋅ 𝐭𝑡
where  𝑠𝑡  and  𝑡𝑡  are  the  beam  thickness  specified  on  either  the  cross  section  or  beam 
element cards.  The rectangular cross-section which contains 𝑠𝑡 and 𝑡𝑡 should completely 
contain  the  cross-sectional  geometry.    Figure  7.4  illustrates  this  for  a  typical  cross-
section.      In  Figure  5.5,  the  area  is  broken  into  twelve  integration  points.    For  each 
integration  point,  it  is  necessary  to  define  the 𝑠  and  𝑡  parametric  coordinates,  (𝑠𝑖,𝑡𝑖),  of 
the centroid of the ith integration point and the relative area associated with the point 
𝐴𝑟𝑖 =
𝐴𝑖
LS-DYNA Theory Manual 
Hughes-Liu Beam 
A1
A2
A3
A4 A5
s6
A12
A11
A10
t6
A6
A7
A8
A9
Figure  7.5.    A  breakdown  of  the  cross  section  geometry  in  Figure  7.4  into
twelve integration points. 
where 𝐴𝑖 is the ratio of the area of the integration point and the actual area of the cross-
section, 𝐴.
LS-DYNA Theory Manual 
Warped Beam Elements 
8    
Warped Beam Elements 
8.1  Resultant Warped Beam 
8.1.1  Green-Lagrange Strains in Terms of Deformational Displacements 
All quantities in this section are referred to the local element coordinate system 
𝐞𝑖, 𝑖 = 1, 2, 3.  The origin of the local system is taken at node 1, with 𝐞1 directed along the 
line  of  centroids,  while  𝐞2,  and  𝐞3  are  directed  along  the  principal  axes  of  the  cross-
section. 
With respect to the local system, the Green-Lagrange strain tensor can be written 
as: 
where, 
𝜀𝑖𝑗 = 𝑒𝑖𝑗 + 𝜂𝑖𝑗,
𝑒𝑖𝑗 = 0.5(𝑢𝑖,𝑗 + 𝑢𝑗,𝑖),
𝜂𝑖𝑗 = 0.5𝑢𝑘,𝑖𝑢𝑘,𝑗.
(8.1)
(8.2)
The  geometric  assumption  of  infinite  in-plane  rigidity  implies 𝜀22 = 𝜀33 = 𝛾23 =
0.  Then the non-zero strain components which contribute to the strain energy are: 
2 + 𝑢2,1
2 + 𝑢3,1
(𝑢1,1
𝜀11 = 𝑢1,1 +
2𝜀12 = 𝑢1,2 + 𝑢2,1 + 𝑢1,1,𝑢1,2 + 𝑢2,1𝑢2,2 + 𝑢3,1𝑢3,2, 
2𝜀13 = 𝑢1,3 + 𝑢3,1 + 𝑢1,1𝑢1,3 + 𝑢2,1𝑢2,3 + 𝑢3,1𝑢3,3.
2 ),
(8.3)
8.1.2  Deformational Displacements After Large Rotations 
The  position  vectors  of  an  arbitrary  point  P  in  the  initial  and  current  local 
configurations are:
Warped Beam Elements 
LS-DYNA Theory Manual 
0 = 𝐱𝐶
𝐱𝑃
0 + [𝐞1
𝐞2
𝐞3]
⎤, 
𝑥2
⎥
𝑥3⎦
⎡
⎢
⎣
𝐱𝑃 = 𝐱𝐶 + [𝐞′1 𝐞′2 𝐞′3]
𝜛𝜙
⎤, 
⎡
𝑥2
⎥
⎢
𝑥3 ⎦
⎣
respectively, with 
where 
[𝐞′1 𝐞′2 𝐞′3] = [𝐈 + 𝛉 +
𝛉2] [𝐞1 𝐞2 𝐞3],
(8.4)
(8.5)
(8.6)
−𝜃3
𝜃1
and  𝜛  is  the  Saint-Venant  warping  function  about  the  centroid  C.    By  the  transfer 
theorem, the following relation holds: 
𝜃2
⎤
−𝜃1
, 
⎥
0 ⎦
⎡
𝜃3
⎢
−𝜃2
⎣
𝛉 =
(8.7)
where 𝜔 refers to the shear center S, and 𝑐2 and 𝑐3 are the coordinates of S. 
𝜛 = 𝜔 + 𝑐2𝑥3 − 𝑐3𝑥2,
(8.8)
Subtracting Equation (8.4) from Equation (8.5) and neglecting third-order terms, 
the displacements vector of point P can be computed: 
𝑢1 = 𝑢̅1 − 𝑥2𝜃3 + 𝑥3𝜃2 +
𝑢2 = 𝑢̅2 − 𝑥3𝜃1 −
u3 = u̅̅̅̅3 + x2θ1 −
2 + 𝜃3
2) +
𝑥2𝜃1𝜃2 +
2) +
x3(θ1
2 + θ2
𝑥2(𝜃1
𝑥3𝜃1𝜃3 + 𝜛𝜙,
𝑥3𝜃2θ3 + 𝜛θ3𝜙, 
x2θ2θ3 − 𝜛θ2𝜙,
(8.9)
where 𝑢̅1, 𝑢̅2, and 𝑢̅3 are the displacements of the centroid C.   
8.1.3  Green-Lagrange Strains in terms of Centroidal Displacements and Angular 
Rotations 
From  Equations  (8.3)  and  (8.9),  a  second-order  approximation  of  the  Green-
2   and  the  nonlinear  strain 
Lagrange  strains  can  be  evaluated.    Neglecting  term  1
components generated by warping, the strain components are simplified as 
2 𝑢1,1
𝜀11 = 𝜀0 + 𝑥2𝜅2 + 𝑥3𝜅3 +
2𝜀12 = 𝛾12 + 𝜛,2𝜙 − 𝑥3𝜅1, 
2𝜀13 = 𝛾13 + 𝜛,3𝜙 + 𝑥2𝜅1,
with 
(𝑥2
2 + 𝑥3
2)𝜃1,1
2 + 𝜔𝜙,1,
(8.10)
LS-DYNA Theory Manual 
Warped Beam Elements 
𝜀0 = 𝑢̅1,1 +
𝜅1 = 𝜃1,1 +
𝜅2 = −𝜃3,1 +
𝜅3 = 𝜃2,1 +
(𝑢̅2,1
2 + 𝑢̅3,1
2 ), 
(𝜃2,1𝜃3 − 𝜃3,1𝜃2), 
(𝜃1𝜃2,1 + 𝜃1,1𝜃2) + 𝑢̅3,1𝜃1,1 − 𝑐3𝜙,1, 
(𝜃1𝜃3,1 + 𝜃1,1𝜃3) − 𝑢̅2,1𝜃1,1 + 𝑐2𝜙,1, 
(8.11)
𝛾12 = 𝑢̅2,1 − 𝜃3 +
𝛾13 = 𝑢̅3,1 + 𝜃2 +
𝜃1𝜃2 + 𝑢̅3,1𝜃1 − 𝑢̅1,1𝜃3, 
𝜃1𝜃3 − 𝑢̅2,1𝜃1 + 𝑢̅1,1𝜃2. 
Numerical  testing  has  shown  that  neglecting  the  nonlinear  terms  in  the  curvatures 𝜅1, 
𝜅2, 𝜅3 and bending shear strains 𝛾12, 𝛾13 has little effect on the accuracy of the results.  
Therefore, Equation (8.11) can be simplified to  
𝜅1 = 𝜃1,1,
𝜀0 = 𝑢̅1,1 +
𝜅2 = −𝜃3,1 − 𝑐3𝜙,1, 𝜅3 = 𝜃2,1 + 𝑐2𝜙,1,
(𝑢̅2,1
2 + 𝑢̅3,1
2 ), 𝛾12 = 𝑢̅2,1 − 𝜃3,
𝛾13 = 𝑢̅3,1 + 𝜃2.
(8.12)
Adopting  Bernoulli’s  assumption  (𝛾12 = 𝛾13 = 0)  and  Vlasov’s  assumption  (𝜙 = θ1,1), 
Equation (8.10) can be rewritten as: 
𝜀11 = 𝜀0 + 𝑥2𝜅2 + 𝑥3𝜅3 +
2𝜀12 = (𝜛,2 − 𝑥3)𝜅1, 
2𝜀13 = (𝜛,3 − 𝑥2)𝜅1,
𝑟2𝜅1
2 + 𝜔𝜃1,11,
where 
𝑟2 = 𝑥2
2 + 𝑥3
2, 𝜅1 = 𝜃1,1, 𝜅2 = −𝑢̅2,11 − 𝑐3𝜃1,11, 𝜅3 = −𝑢̅3,11 + 𝑐2𝜃1,11. 
To avoid membrane locking, ε11 in Equation (8.13) is reformulated as 
𝜀11 = 𝜀𝑎 + 𝑥2𝜅2 + 𝑥3𝜅3 +
2 + 𝜔𝜃1,11,
(𝑟2 −
) 𝜅1
𝐼𝑜
where 
𝜀𝑎 =
∫ [𝑢̅1,1 +
8.1.4  Strain Energy 
(𝑢̅2,1
2 + 𝑢̅3,1
2 +
𝐼𝑜
2)] 𝑑𝑥1
𝜅1
.
(8.13)
(8.14)
(8.15)
(8.16)
Assuming material is linear elastic, the strain energy can be evaluated from:
2 𝑑𝐴
∫ 𝜀11
with 
Warped Beam Elements 
LS-DYNA Theory Manual 
𝑈 = ∫ (
2 𝑑𝐴 +
𝐸 ∫ 𝜀11
𝐺 ∫ [(2𝜀12)2 + (2𝜀13)2]𝑑𝐴
)
𝑑𝑥1. 
(8.17)
The following relations are used in integrating the previous equations:   
(1) Since the reference frame is located at centroid C with e2 and e3 directed along the 
principal axes, 
∫ 𝑥2𝑑𝐴 = 0
,
∫ 𝑥3𝑑𝐴 = 0
,
∫ 𝑥2𝑥3𝑑𝐴 = 0
.
(2) Since sectorial area ω refers to shear center S, 
∫ 𝜔𝑑𝐴 = 0
,
∫ 𝑥2𝜔𝑑𝐴 = 0
,
∫ 𝑥3𝜔𝑑𝐴 = 0
.
Integration through the cross-section gives: 
+ 𝐴𝜀𝑎
2 + 𝐼22𝜅2
2 + 𝐼𝜔𝜃1,11
2 + 𝐼2𝑟𝜅2𝜅1
2 + 𝐼3𝑟𝜅3𝜅1
2 + 𝐼𝜔𝑟𝜃1,11𝜅1
2 + 𝐼33𝜅3
𝐼𝑜
4 
) 𝜅1
+
(𝐼𝑟𝑟 −
∫ [(2ε12)2 + (2ε13)2]
2 
dA = 𝐽κ1
𝐼33 = ∫ 𝑥3
2𝑑𝐴
,
𝐼3𝑟 = ∫ 𝑥3𝑟2𝑑𝐴,
𝐼𝜔𝑟 = ∫ 𝜔𝑟2𝑑𝐴
,
𝐼𝑂 = 𝐼22 + 𝐼33
𝐼𝑟𝑟 = ∫ 𝑟4𝑑𝐴
𝐽 = ∫ [(𝜔̅̅̅̅,3 + 𝑥2)2 + (𝜔̅̅̅̅,2 − 𝑥3)2]
𝑑𝐴
𝐼22 = ∫ 𝑥2
2𝑑𝐴
,
𝐼2𝑟 = ∫ 𝑥2𝑟2𝑑𝐴,
𝐼𝜔 = ∫ 𝜔2𝑑𝐴
,
6.1.5  Displacement Field 
Linear  interpolation  is  used  for  axial  displacement  𝐮̅̅̅̅,  whereas  Hermitian 
interpolations  are  used  for  𝑢2,  𝑢3,  and  𝜃1,  considering  the  following  relations  used  in 
deriving the final expression of strain energy: 
𝜃2 = −𝑢3,1 𝜃3 = 𝑢2,1 𝜙 = 𝜃1,1.
The nodal displacement field is constructed by 
𝑢̅1 = 𝐍1𝐝,
(8.23)
(8.24)
8-4 (Warped Beam Elements) 
LS-DYNA Draft 
(8.18)
(8.19)
(8.20)
LS-DYNA Theory Manual 
Warped Beam Elements 
{⎧𝑢̅2
}⎫
𝑢̅3
𝜃1 ⎭}⎬
⎩{⎨
= 𝐍2𝐝, 
(8.25)
where 
𝐝T = [0
𝜃2𝐼
𝜃3𝐼 𝜙𝐼 𝑢̅1𝐽𝐼
𝜃1𝐽𝐼
𝜃2𝐽
𝜃3𝐽 𝜙𝐽]T, 
(8.26)
𝐍1 = [1 − 𝜉 ⋅⋅⋅⋅⋅⋅|    𝜉 ⋅          ⋅  
⋅
∣       ⋅   1 − 𝑓           ⋅            ⋅   ⋅    ℎ    ⋅
⋅ 𝑓          ⋅  ⋅   ⋅    𝑔    ⋅
∣∣∣
      ⋅  ⋅     1 − 𝑓           ⋅      −ℎ      ⋅       ⋅
⋅⋅         𝑓    ⋅      −𝑔     ⋅   ⋅
⋅
⋅⋅         ⋅   𝑓        ⋅      ⋅  𝑔∣
1 − 𝑓
⋅ ],
⋅
⋅
⋅
⋅
⋅
𝐍2 =
⎡
⎢
⎣
with 
𝑓 = 1 − 3𝜉 2 + 2𝜉 3𝑔 = 𝑙(𝜉 − 2𝜉 2 + 𝜉 3)ℎ = 𝑙(𝜉 3 − 𝜉 2).
Equations (8.25) and (8.27) also imply 
𝜃1,1 = 𝐍3𝐝,
where 
𝐍3 = [⋅⋅ 𝑓,1 ⋅⋅ 𝑔,1∣ ⋅⋅⋅ −𝑓,1 ⋅⋅ ℎ,1].
⎤
, 
⎥
  ⋅           ℎ⎦
(8.27)
(8.28)
(8.29)
(8.30)
6.1.6  Strain Energy in Matrix Form 
The strain energy due to the average strain εa defined in Equation (8.16) can be 
expressed in matrix form as  
𝑈1 =
where 
𝐸𝐴𝑙 [∫ (𝐍1,1𝐝)𝑑𝜉 +
𝐝T [∫ (𝐍2,1
T 𝐃𝐍2,1)𝑑𝜉
] 𝐝
]
, 
𝐃 = diag (1,1,
𝐼𝑜
).
The strain energy due to the second through fourth terms is 
𝑈2 =
𝐸𝑙𝐝T [∫ 𝐍2,11
T 𝐇𝐍2,11𝑑𝜉
] 𝐝,
(8.31)
(8.32)
(8.33)
where 
𝐇 =
𝐼22   
⎡
⎢
𝐼22𝑐3  −𝐼33𝑐2
⎣
𝐼33
𝐼22𝑐3
−𝐼33𝑐2
𝐼′𝜔
⎤
⎥
⎦
,
𝐼′𝜔 = 𝐼𝜔 + 𝐼22𝑐3
2. 
2 + 𝐼33𝑐2
(8.34)
The strain energy due to the fifth through seventh terms is
Warped Beam Elements 
LS-DYNA Theory Manual 
𝑈3 =
𝐸𝑙 [∫ (𝐍3𝐝)2
𝛖𝐍2,11𝑑𝜉 ] 𝐝,
where 
𝛖 = (−𝐼2𝑟        − 𝐼3𝑟 
𝐼′𝜔𝑟),
𝐼′𝜔𝑟 = 𝐼𝜔𝑟 − 𝑐3𝐼2𝑟 + 𝑐2𝐼3𝑟. 
The strain energy due to the eighth and ninth terms is 
𝑈4 =
𝐸𝑙 (𝐼𝑟𝑟 −
𝐼𝑜
) ∫ (𝐍3𝐝)4𝑑𝜉 +
𝐺𝐽𝑙 ∫ (𝐍3𝐝)2𝑑𝜉
(8.35)
(8.36)
(8.37)
6.1.7  Internal Nodal Force Vector 
The internal force can be evaluated from 
𝐟e = 𝐸𝐴𝑙 (
𝐮̅̅̅̅1𝐽𝐿
+
𝐝T𝐐) (𝐏 + 𝐐) + 𝐸 (𝐑 +
𝐒 + 𝐓 +
𝐕) + G𝐖, 
(8.38)
where 
𝐏 = ∫ 𝐍1,1
T 𝑑𝜉
,        𝐐 = [∫ 𝐍2,1
𝐒 = l [∫ (𝐍3𝐝)2
𝐍2,11
T 𝑑𝜉  ] 𝛖T,    𝐓 = 𝑙 ∫ (𝐍3𝐝)(𝛖𝐍2,11𝐝)
𝐃𝐍2,1𝑑𝜉 ] 𝐝,
T 𝐇𝐍2,11𝑑𝜉
𝐑 = l [∫ 𝐍2,11
T𝑑𝜉 ,
𝐍3
] 𝐝,
(8.39)
𝐕 = (𝐼𝑟𝑟 −
𝐼𝑜
) l ∫ (𝐍3𝐝)3𝐍3
T𝑑𝜉
,
𝐖 = 𝐽𝑙 ∫ (𝐍3𝐝)𝐍3
T𝑑𝜉
,
𝜆 =
𝑢̅1𝐽𝐼
+
𝐝T𝐐.
With  respect  to  the  local  coordinate  system,  there  are  totally  eight  independent 
components  in  the  nodal  force  vector,  in  correspondence  to  the  eight  nodal 
displacement components.   
Other forces can be calculated by: 
𝐅1 = −𝐅8,      𝐅2 =
 𝐅4 = −𝐅11,      𝐅9 = −𝐅2,
𝐅6 + 𝐅13
,
𝐅5 + 𝐅12
𝐅3 = −
𝐅10 = −𝐅3.
,
(8.40)
6.2  Integrated Warped Beam 
6.2.1  Kinematics 
We introduce three coordinate systems that are mutually interrelated.  The first 
coordinate system is the orthogonal Cartesian coordinate system (𝑥, 𝑦, 𝑧), for which the 
y  and  zaxes  lie  in  the  plane  of  the  cross-section  and  the  𝑥-axis  parallel  to  the 
longitudinal  axis  of  the  beam.    The  second  coordinate  system  is  the  local  plate 
coordinate  system  (𝑥, 𝑠, 𝑛)  as  shown  in  Figure  6.1,  wherein  the  n-axis  is  normal  to  the 
middle  surface  of  a  plate  element,  the  s-axis  is  tangent  to  the  middle  surface  and  is 
directed along the contour line of the cross-section.  The (𝑥, 𝑠, 𝑛) and (𝑥, 𝑦, 𝑧) coordinate
LS-DYNA Theory Manual 
Warped Beam Elements 
systems are related through an angle of orientation 𝜃 as defined in Figure 40.1. The third 
coordinate set is the contour coordinate s along the profile of the section with its origin 
at some point O on the profile section.  Point P is called the pole through which the axis 
parallel to the x-axis is  called the pole axis.  To derive the analytical model for a thin-
walled beam, the following two assumptions are made: 
1.  The contour of the thin wall does not deform in its own plane. 
2.  The shear strain γsx of the middle surface is zero. 
According  to  assumption  1,  the  midsurface  displacement  components  𝑣  and  𝑤 
with respect to the (𝑥, 𝑠, 𝑛) coordinate system at a point A can be expressed in terms of 
displacements 𝐕 and 𝐖 of the pole P in the (𝑥, 𝑦, 𝑧) coordinate system and the rotation 
angle 𝜙𝑥 about the pole axis 
𝐯(𝑥, 𝑠) = 𝐕(𝑥)cos𝜃(𝑠) + 𝐖(𝑥)sin𝜃(𝑠) − 𝐫(𝑠)ϕ𝑥(𝑥),
𝐰(𝑥, 𝑠) = −𝐕(𝑥)sin𝜃(𝑠) + 𝐖(𝑥)cos𝜃(𝑠) − 𝐪(𝑠)ϕ𝑥(𝑥).
(8.41)
These  equations  apply  to  the  whole  contour.    The  out-of-plane  displacement  u 
can now be found from assumption 2. On the middle surface 
∂𝐮
∂𝑠
+
∂𝐯
∂𝑥
= 𝟎,
which can be written 
∂𝐮
∂s
= −
∂𝐯
∂𝑥
= −𝐕′(𝑥)cos𝜃(𝑠) − 𝐖′(𝑥)sin𝜃(𝑠) + 𝐫(𝑠)ϕ′𝑥(𝑥). 
(8.42)
(8.43)
Integrating this relation from point O to an arbitrary point on the contour yields 
(using t as a dummy for s) 
q(s)
θ(s)
r(s)
Figure 8.1.  Definition of coordinates in thin-walled open section
Warped Beam Elements 
LS-DYNA Theory Manual 
∫
∂𝐮
∂𝑡
𝑑𝑡
= −𝐕′(𝑥) ∫ cos𝜃(𝑡)𝑑𝑡
− 𝐖′(𝑥) ∫ sin𝜃(𝑡)𝑑𝑡
+ ϕ′𝑥(𝑥) ∫ 𝐫(𝑡)𝑑𝑡
. 
Noting that 
we end up with 
𝑑𝑦 = cos𝜃(𝑡)𝑑𝑡,
𝑑𝑧 = sin𝜃(𝑡)𝑑𝑡.
𝑢(𝑥, 𝑠) = 𝑢(𝑥, 0) + V′(𝑥)𝑦(0) + W′(𝑥)𝑧(0) + ϕ′𝑥(𝑥)ϖ
⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟
=:𝐔(𝑥)
              − 𝑉′(𝑥)⏟
=:𝜙𝑧(𝑥)
𝑦(𝑠) − W′(𝑥)⏟
=:−𝜙𝑦(𝑥)
             = 𝑈(𝑥) − 𝜙𝑧(𝑥)𝑦 + 𝜙𝑦(𝑥)𝑧 + 𝜙′𝑥(𝑥)(𝜔(𝑠) − ϖ).
z(𝑠) + ϕ′𝑥(𝑥)(ω(𝑠) − ϖ)
(8.44)
(8.45)
(8.46)
where  𝑈  denotes  the  average  out-of-plane  displacement  over  the  section,  𝜙𝑦  and  𝜙𝑧 
denote  the  rotation  angle  about  the  y  and  z  axis1,  respectively,  ω  is  the  sectorial  area 
defined as 
𝜔(𝑠) = ∫ 𝑟(𝑡)𝑑𝑡
,
and ϖ is the average of the sectorial area over the section. 
The expression for the displacements in the (x, y, z) coordinate system is 
𝑢(𝑥, 𝑦, 𝑧) = 𝑈(𝑥) − 𝜙𝑧(𝑥)𝑦 + 𝜙𝑦(𝑥)𝑧 + 𝜗(𝑥)𝜔(𝑦, 𝑧),
𝑣(𝑥, 𝑦, 𝑧) = 𝑉(𝑥) − 𝜙𝑥(𝑥)𝑧, 
𝑤(𝑥, 𝑦, 𝑧) = 𝑊(𝑥) + 𝜙𝑥(𝑥)𝑦,
where we have introduced ϑ to represent the twist constrained by the condition 
𝜗(𝑥) = 𝜙𝑥(𝑥).
(8.47)
(8.48)
(8.49)
and 𝜔 denotes the sectorial coordinate that is adjusted for zero average over the section. 
6.2.2  Kinetics 
The kinetic energy of the beam can be written 
𝑇 =
∫ 𝜌{𝑢̇2 + 𝑣̇2 + 𝑤̇ 2}
𝑑𝑉.
(8.50)
Taking the variation of this expression leads to  
1  The  substitution  of  𝑉′(𝑥)  for  𝜙(cid:3053)(𝑥)  and  𝑊′(𝑥)  for  −𝜙(cid:3052)(𝑥)  can  be  seen  as  a  conversion  from  an  Euler-
Bernoulli kinematic assumption to that of Timoschenko.
LS-DYNA Theory Manual 
Warped Beam Elements 
δT = ∫ ρ{u̇δu̇ + v̇δv̇ + ẇ δẇ }
dV
       = ∫ ρ{U̇ − 𝜙̇zy + 𝜙̇yz + 𝜗̇ω}{δU̇ − δ𝜙̇zy + δ𝜙̇yz + δ𝜗̇ω}dV
+
           ∫ ρ{V̇ − 𝜙̇xz}{δV̇ − δ𝜙̇xz}dV
+ ∫ ρ{Ẇ + 𝜙̇xy}{δẆ + δ𝜙̇xy}dV
       = ∫ ρ{U̇ δU̇ + y2𝜙̇zδ𝜙̇z − yω𝜙̇zδ𝜗̇ + z2𝜙̇yδ𝜙̇y}dV
+
           ∫ ρ{zω𝜙̇yδ𝜗̇ − yω𝜗̇δ𝜙̇z + zω𝜗̇δ𝜙̇y + ω2𝜗̇δ𝜗̇}dV
+
(8.51)
           ∫ ρ{V̇ δV̇ + z2𝜙̇xδ𝜙̇x + Ẇ δẆ + y2𝜙̇xδ𝜙̇x}dV
       = ρA ∫{U̇ δU̇ + V̇ δV̇ + Ẇ δẆ }dV
+ ρIzz ∫{𝜙̇zδ𝜙̇z + 𝜙̇xδ𝜙̇x}dV
+
            ρIýy ∫{𝜙̇yδ𝜙̇y + 𝜙̇xδ𝜙̇x}dV
+ ρIyω ∫{𝜙̇yδ𝜗̇ + 𝜗̇δ𝜙̇y}dV
−
           ρIzω ∫{𝜗̇δ𝜙̇z + 𝜙̇zδ𝜗̇}dV + ρIωω ∫ 𝜗̇δ𝜗̇dV
,
from  which  the  consistent  mass  matrix  can  be  read  out.    Here A  is  the  cross  sectional 
area,  Izz  and  Iyy  are  the  second  moments  of  area  with  respect  to  the  z  and  y  axes, 
respectively,  Iωω  is  the  sectorial  second  moment  and  Izω  and  Iyω  are  the  sectorial 
product  moments.    An  approximation  of  this  mass  matrix  can  be  made  by  neglecting 
the off diagonal components.  The diagonal components are 
𝑚TRNS =
𝜌𝐴𝑙
, 
, 
(8.52)
𝜌(𝐼𝑦𝑦 + 𝐼𝑧𝑧)𝑙
𝑚RT𝑥 =
𝑚RT𝑦 =
𝑚RT𝑧 =
𝑚TWST =
, 
𝜌𝐼𝑦𝑦𝑙
𝜌𝐼𝑧𝑧𝑙
𝜌𝐼𝜔𝜔𝑙
, 
. 
With 𝐸 as Young’s modulus and 𝐺 as the shear modulus, the strain energy can be 
written
Warped Beam Elements 
LS-DYNA Theory Manual 
𝛱 =
(𝐸𝜀𝑥𝑥
2 + 𝐺𝛾𝑥𝑦
2 + 𝐺𝛾𝑥𝑧
2 ),
(8.53)
where  the  infinitesimal  strain  components  are  (neglecting  the  derivatives  of  sectorial 
area) 
′ 𝑦 + 𝜗′𝜔,
𝜀𝑥𝑥 = 𝑈′ + 𝜙𝑦
𝛾𝑥𝑦 = 𝑉′ − 𝜙𝑥
𝛾𝑥𝑧 = 𝑊′ + 𝜙𝑥
′ 𝑧 − 𝜙𝑧
′ 𝑧 − 𝜙𝑧, 
′ 𝑦 + 𝜙𝑦.
and the variation of the same can be written 
𝛿𝜀𝑥𝑥 = 𝛿𝑈′ + 𝛿𝜙𝑦
𝛿𝛾𝑥𝑦 = 𝛿𝑉′ − 𝛿𝜙𝑥
𝛿𝛾𝑥𝑧 = 𝛿𝑊′ + 𝛿𝜙𝑥
′ 𝑧 − 𝛿𝜙𝑧
′ 𝑧 − 𝛿𝜙𝑧, 
′ 𝑦 + 𝛿𝜙𝑦.
′ 𝑦 + 𝛿𝜗′𝜔,
The variation of the strain energy is 
𝛿𝛱 = ∫{𝐸𝜀𝑥𝑥𝛿𝜀𝑥𝑥 + 𝐺𝛾𝑥𝑦𝛿𝛾𝑥𝑦 + 𝐺𝛾𝑥𝑧𝛿𝛾𝑥𝑧}𝑑𝑉
       = 𝐸𝐴 ∫ 𝑈′𝛿𝑈′𝑑𝑙
+ 𝐺𝐴 ∫ 𝑉′𝛿𝑉′𝑑𝑙
           𝐸𝐼𝑦𝑦 ∫ 𝜙𝑦
′ 𝛿𝜙𝑦
′ 𝑑𝑙
+ 𝐺𝐴 ∫ 𝜙𝑦𝛿𝜙𝑦𝑑𝑙
           𝐸𝐼𝜔𝜔 ∫ 𝜗′𝛿𝜗′𝑑𝑙
− 𝐺𝐴 ∫(𝑉′𝛿𝜙𝑧 + 𝜙𝑧𝛿𝑉′)𝑑𝑙
+  𝐺𝐴 ∫ 𝑊′𝛿𝑊′𝑑𝑙
+ 𝐺(𝐼𝑦𝑦 + 𝐼𝑧𝑧) ∫ 𝜙𝑥
′ 𝛿𝜙𝑥
′ 𝑑𝑙
+ 𝐸𝐼𝑧𝑧 ∫ 𝜙𝑧
′ 𝑑𝑙
′ 𝛿𝜙𝑧
+ 𝐺𝐴 ∫ 𝜙𝑧𝛿𝜙𝑧𝑑𝑙
+ 𝐺𝐴 ∫(𝑊′𝛿𝜙𝑦 + 𝜙𝑦𝛿𝑊′)𝑑𝑙
+
+
(8.54)
(8.55)
+
  (8.56)
            𝐸𝐼𝑦𝜔 ∫(𝜙𝑦
′ )𝑑𝑙
′ 𝛿𝜗′ + 𝜗′𝛿𝜙𝑦
−  𝐸𝐼𝑧𝜔 ∫(𝜙𝑧
′ 𝛿𝜗′ + 𝜗′𝛿𝜙𝑧
′ )𝑑𝑙
,
where the stiffness matrix can be read.  Again the diagonal components are
LS-DYNA Theory Manual 
Warped Beam Elements 
𝑘TRNS =
𝑘SHR =
𝑘RTx =
𝑘RTy =
𝑘RTz =
, 
𝐸𝐴
𝐺𝐴
, 
𝐺(𝐼𝑦𝑦 + 𝐼𝑧𝑧)
𝐺𝐴𝑙
𝐺𝐴𝑙
, 
, 
+
𝐸𝐼𝑦𝑦
𝐸𝐼𝑧𝑧
+
𝐸𝐼𝜔𝜔
𝑘TWST =
. 
, 
(8.57)
From  the  expressions  of  the  mass  and  stiffness  matrix,  the  frequencies  of  the 
most common modes can be estimated.  These are 
1.  The tensile and twisting modes with frequency 𝜔 =
√3
√𝐸
𝜌. 
2.  The transverse shear and torsional mode with frequency 𝜔 =
3.  The bending modes with frequencies 𝜔 = √3𝐸
𝜌𝑙2 + 𝐺𝐴
𝜌𝐼𝑦𝑦
 and 𝜔 = √3𝐸
√3
√𝐺
𝜌. 
𝜌𝑙2 + 𝐺𝐴
𝜌𝐼𝑧𝑧
. 
Which one of these four that is the highest depends on the geometry of the beam 
element.  In LS-DYNA the first of these frequencies is used for calculating a stable time 
step.  We have found no reason for changing approach regarding this element. 
6.2.3  Penalty on Twist 
The twist is constrained using a penalty that is introduced in the strain energy as 
𝛱P =
𝑃𝐸A
′ − 𝜗)2𝑑𝑙
∫(𝜙𝑥
,
and the corresponding variation is 
𝛿𝛱 = 𝑃𝐸𝐴 ∫(𝜙𝑥
′ − 𝜗)(𝛿𝜙𝑥
′ − 𝛿𝜗)𝑑𝑙
(8.58)
(8.59)
.
The diagonal of the stiffness matrix is modified as follows
Warped Beam Elements 
LS-DYNA Theory Manual 
𝑘RTx =
𝑘TWST =
+
𝐺(𝐼𝑦𝑦 + 𝐼𝑧𝑧)
𝐸𝐼𝜔𝜔
+
𝑃𝐸𝐴𝑙
𝑃𝐸𝐴
, 
. 
(8.60)
This increases the twist mode frequency to √3𝐸
𝜌𝑙2 + 𝑃𝐸𝐴
𝜌𝐼𝜔𝜔
 and the torsional mode to  
√3
√
𝐺(𝐼𝑦𝑦 + 𝐼𝑧𝑧) + 𝑃𝐸𝐴
.
(8.61)
Even  though  this  gives  an  indication  of  a  frequency  increase  we  have  made  no 
modifications  on  the  computation  of  the  critical  time  step  in  an  explicit  analysis.    We 
have  used  𝑃 = 1  in  the  implementation.    This  decision  may  have  to  be  reconsidered 
depending on the choice of the parameter 𝜇, in the end it will come down to trial and 
error from numerical simulations. 
6.3  Generalization to Large Displacements 
A  generalization  of  the  small  displacement  theory  to  nonlinear  theory  is  quite 
straightforward.    We  have  used  a  corotational  formulation  where  the  small  strains  in 
the linear theory are used directly as strain rates in the element system.  We emphasize 
that the nonlinear beam formulation is obtained by simply replacing displacements for 
velocities and strains with strain rates in the previous section.  
The nodal velocities for a beam element in the local system is written  
𝐯 = (𝑣𝑥
𝑣𝑦
1 𝜔𝑥
𝑣𝑧
1 𝜔𝑦
1 𝜔𝑧
1 𝜗̇1
𝑣𝑥
𝑣𝑦
2 𝜔𝑥
𝑣𝑧
2 𝜔𝑦
2 𝜔𝑧
2 𝜗̇2)
, 
(8.62)
where  the  superscript  refers  to  the  local  node  number.    These  are  obtained  by 
transforming  the  translational  velocities  and  rotational  velocities  using  the  local  to 
global transformation matrix qij. The strain rate – velocity matrix in the local system can 
be written 
𝐁0 = 
−1
−𝑙0
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
−
−𝑙0
−1𝑧
−1
−1𝜔 𝑙0
−1𝑦 −𝑙0
𝑙0
−𝑙0
−1𝑧
𝑙0
−1
−𝑙0
−1 −𝑙0
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
2 ⎦
where  𝑙0  is  the  beam  length  in  the  reference  configuration,  i.e.,  beginning  of  the  time 
step.  A corresponding matrix w.r.t. the current configuration is 
−1
−𝑙0
−1𝑦
𝑙0
−1𝑦
−1
𝑙0
−1
𝑙0
−1
𝑙0
−𝑙0
−1𝑧 −𝑙0
−1𝑦
𝑙0
−1𝑧 0
−1𝜔
𝑙0
−
−
−
,(8.63)
LS-DYNA Theory Manual 
Warped Beam Elements 
𝐁 = 
−𝑙−1
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
−𝑙−1𝑧 −𝑙−1𝑦 −𝑙−1𝜔 𝑙−1
𝑙−1𝑧 −𝑙−1𝑦
𝑙−1𝜔
−
𝑙−1
𝑙−1𝑧
−𝑙−1
−𝑙−1 −𝑙−1𝑦
⎤
⎥
⎥
⎥
(8.64)
,
⎥
⎥
⎥
⎥
2 ⎦
where  we  use  the  current  length  of  the  beam.    These  matrices  are  evaluated  in  each 
integration  point  (𝑥, 𝑦)  of  the  cross  section.    To  compute  the  strain  rate  in  the  local 
system we simply apply 
−𝑙−1𝑧 0
−𝑙−1
𝑙−1𝑦
𝑙−1
𝑙−1
−
−
−
which  is  then  used  to  update  the  local  stresses  𝛔.  The  internal  force  vector  is  then 
assembled as 
𝛆̇ = 𝐁0𝐯,
(8.65)
𝐟 = 𝐁T𝛔.
(8.66)
Finally  the  internal  force  is  transformed  to  the  global  system  using  the 
transformation matrix.  
To  compute  the  stiffness  matrix  for  implicit  we  neglect  the  geometric 
contribution and just apply  
where 𝐂 is the material tangent modulus.  Again the matrix must be transformed to the 
global system before used in the implicit solver.
𝐊 = 𝐁T𝐂𝐁,
(8.67)
LS-DYNA Theory Manual 
Belytschko-Lin-Tsay Shell 
9    
Belytschko-Lin-Tsay Shell 
The Belytschko-Lin-Tsay shell element ([Belytschko and Tsay 1981], [Belytschko 
et al., 1984a]) was implemented in LS-DYNA as a computationally efficient alternative 
to  the  Hughes-Liu  shell  element.    For  a  shell  element  with  five  through  thickness 
integration  points,  the  Belytschko-Lin-Tsay  shell  elements  requires  725  mathematical 
operations compared to 4050 operations for the under integrated Hughes-Liu element.  
The  selectively  reduced  integration  formulation  of  the  explicit  Hughes-Liu  element 
requires  35,350  mathematical  operations.    Because  of  its  computational  efficiency,  the 
Belytschko-Lin-Tsay  shell  element  is  usually  the  shell  element  formulation  of  choice.  
For  this  reason,  it  has  become  the  default  shell  element  formulation  for  explicit 
calculations. 
The Belytschko-Lin-Tsay shell element is based on a combined co-rotational and 
velocity-strain  formulation.    The  efficiency  of  the  element  is  obtained  from  the 
mathematical simplifications that result from these two kinematical assumptions.  The 
co-rotational portion of the formulation avoids the complexities of nonlinear mechanics 
by embedding a coordinate system in the element.  The choice of velocity-strain or rate-
of-deformation  in  the  formulation  facilitates  the  constitutive  evaluation,  since  the 
conjugate  stress  is  the  physical  Cauchy  stress.    We  closely  follow  the  notation  of 
Belytschko, Lin, and Tsay in the following development. 
9.1  Co-rotational Coordinates 
The midsurface of the quadrilateral shell element, or reference surface, is defined 
by  the  location  of  the  element’s  four  corner  nodes.    An  embedded  element  coordinate 
system  that deforms with the element is defined in terms of these nodal 
coordinates.    Then  the  procedure  for  constructing  the  co-rotational  coordinate  system 
begins by calculating a unit vector normal to the main diagonal of the element:
Belytschko-Lin-Tsay Shell 
LS-DYNA Theory Manual 
y^
e^
r42
e^
s3
e^
r31
s1
x^
r21
Figure 9.1.  Construction of element coordinate system is shown. 
𝐞̂3 =
𝐬3
∥𝐬3∥
,
∥𝐬3∥ = √[𝐬3]1
2 + [𝐬3]2
2,
2 + [𝐬3]3
𝐬3 = 𝐫31 × 𝐫42,
(9.1)
(9.2)
(9.3)
where the superscript caret (⋅ ̂) is used to indicate the local (element) coordinate system. 
It is desired to establish the local 𝑥 axis 𝑥̂ approximately along the element edge 
between  nodes  1  and  2.    This  definition  is  convenient  for  interpreting  the  element 
stresses,  which  are  defined  in  the  local  𝑥̂ − 𝑦̂  coordinate  system.    The  procedure  for 
constructing this unit vector is to define a vector 𝐬1 that is nearly parallel to the vector 
𝐫21, viz. 
𝐬1 = 𝐫21 − (𝐫21 ⋅ 𝐞̂3)𝐞̂3,
𝐞̂1 =
𝐬1
‖𝐬1‖
.
The remaining unit vector is obtained from the vector cross product 
𝐞̂2 = 𝐞̂3 × 𝐞̂1.
(9.4)
(9.5)
(9.6)
If the four nodes of the element are coplanar, then the unit vectors 𝐞̂1 and 𝐞̂2 are 
tangent  to  the  midplane  of  the  shell  and  𝐞̂3  is  in  the  fiber  direction.    As  the  element 
deforms, an angle may develop between the actual fiber direction and the unit normal 
𝐞̂3.  The magnitude of this angle may be characterized as 
9-2 (Belytschko-Lin-Tsay Shell) 
∣𝐞̂3 ⋅ 𝐟 − 1∣ < 𝛿,
LS-DYNA Theory Manual 
Belytschko-Lin-Tsay Shell 
where 𝐟 is the unit vector in the fiber direction and the magnitude of 𝛿 depends on the 
magnitude  of  the  strains.    According  to  Belytschko  et  al.,  for  most  engineering 
applications,  acceptable  values  of  𝛿  are  on  the  order  of  10-2  and  if  the  condition 
presented  in  Equation  (9.7)  is  met,  then  the  difference  between  the  rotation  of  the  co-
rotational coordinates 𝑒 ̂ and the material rotation should be small. 
The global components of this co-rotational triad define a transformation matrix 
between the global and local element coordinate systems.  This transformation operates 
on  vectors  with  global  components  𝐀 = (𝐴𝑥 𝐴𝑦 𝐴𝑧)  and  element  coordinate 
components 𝐀̂ = (𝐴̂𝑥 𝐴̂𝑦 𝐴̂𝑧), and is defined as:  
⎧𝐴̂𝑥
⎫
}}
{{
𝐴̂𝑦
⎬
⎨
}}
{{
𝐴̂𝑧⎭
⎩
{⎧𝐴𝑥
}⎫
𝐴𝑦
𝐴𝑧⎭}⎬
⎩{⎨
= 𝛍𝐀̂ = 𝐪T𝐀̂, 
𝑒3𝑥
⎥⎤
𝑒3𝑦
𝑒3𝑧⎦
𝑒1𝑥
⎢⎡
𝑒1𝑦
𝑒1𝑧
⎣
𝑒2𝑥
𝑒2𝑦
𝑒2𝑧
𝐀 =
=
(9.8)
where 𝑒𝑖𝑥, 𝑒𝑖𝑦, 𝑒𝑖𝑧  are the global components of the element coordinate unit vectors.  The 
inverse transformation is defined by the matrix transpose, i.e., 
𝐀̂ = 𝛍T𝐀.
(9.9)
9.2  Velocity-Strain Displacement Relations 
The  above  small  rotation  condition,  Equation  (9.7),  does  not  restrict  the 
magnitude of the element’s rigid body rotations.  Rather, the restriction is placed on the 
out-of-plane  deformations,  and,  thus,  on  the  element  strain.    Consistent  with  this 
restriction  on  the  magnitude  of  the  strains,  the  velocity-strain  displacement  relations 
used in the Belytschko-Lin-Tsay shell are also restricted to small strains. 
As in the Hughes-Liu shell element, the displacement of any point in the shell is 
partitioned  into  a  midsurface  displacement  (nodal  translations)  and  a  displacement 
associated with rotations of the element’s fibers (nodal rotations).  The Belytschko-Lin-
Tsay  shell  element  uses  the  Mindlin  [1951]  theory  of  plates  and  shells  to  partition  the 
velocity of any point in the shell as: 
(9.10)
where 𝐯 𝑚 is the velocity of the mid-surface, 𝛉 is the angular velocity vector, and 𝑧̂ is the 
distance  along  the  fiber  direction  (thickness)  of  the  shell  element.    The  corresponding 
co-rotational components of the velocity strain (rate of deformation) are given by 
𝐯 = 𝐯 𝑚 − 𝑧̂ 𝐞3 × 𝛉,
𝑑 ̂
𝑖𝑗 =
(
∂𝜐̂𝑖
∂𝑥̂𝑗
+
∂𝜐̂𝑗
∂𝑥̂𝑖
).
(9.11)
Substitution  of  Equation  (9.10)  into  the  above  yields  the  following  velocity-strain 
relations:
Belytschko-Lin-Tsay Shell 
LS-DYNA Theory Manual 
𝑑 ̂
𝑥 =
𝑑 ̂
𝑦 =
∂𝑣̂𝑥
∂𝑥̂
∂𝜐̂𝑦
∂𝑦̂
+ 𝑧̂
− 𝑧̂
∂ 𝜃̂
∂𝑥̂
,
∂ 𝜃̂
∂𝑦̂
,
2𝑑 ̂
𝑥𝑦 =
∂𝜐̂𝑥
∂𝑦̂
+
∂𝜐̂𝑦
∂𝑥̂
+ 𝑧̂
∂ 𝜃̂
∂𝑦̂
⎜⎛
⎝
−
∂ 𝜃̂
⎟⎞,
∂𝑥̂ ⎠
2𝑑 ̂
𝑦𝑧 =
2𝑑 ̂
𝑥𝑧 =
∂𝜐̂𝑧
∂𝑦̂
∂𝜐̂𝑧
∂𝑥̂
− 𝜃̂
𝑥,
+ 𝜃̂
𝑦.
(9.12)
(9.13)
(9.14)
(9.15)
(9.16)
The above velocity-strain relations need to be evaluated at the quadrature points 
within the shell.  Standard bilinear nodal interpolation is used to define the mid-surface 
velocity, angular velocity, and the element’s coordinates (isoparametric representation).  
These interpolations relations are given by 
𝐯𝑚 = 𝑁𝐼(𝜉 , 𝜂)𝐯𝐼,
𝛉𝑚 = 𝑁𝐼(𝜉 , 𝜂)𝛉𝐼, 
𝐱𝑚 = 𝑁𝐼(𝜉 , 𝜂)𝐱𝐼.
(9.17)
where  the  subscript  𝐼  is  summed  over  all  the  nodes  of  the  element  and  the  nodal 
velocities are obtained by differentiating the nodal coordinates with respect to time, i.e., 
𝜐𝐼 = 𝑥̇𝐼.  The bilinear shape functions are 
𝑁1 =
𝑁2 =
𝑁3 =
𝑁4 =
(1 − 𝜉 )(1 − 𝜂),
(1 + 𝜉 )(1 − 𝜂),
(1 + 𝜉 )(1 + 𝜂),
(1 − 𝜉 )(1 + 𝜂).
(9.18)
(9.19)
(9.20)
(9.21)
The  velocity-strains  at  the  center  of  the  element,  i.e.,  at  𝜉 = 0,  and  𝜂 = 0,  are 
obtained  by  substitution  of  the  above  relations  into  the  previously  defined  velocity-
strain  displacement  relations,  Equations  (9.12)  and  (9.16).    After  some  algebra,  this 
yields 
𝑑 ̂
𝑥 = 𝐵1𝐼𝜐̂𝑥𝐼 + 𝑧̂𝐵1𝐼𝜃̂
𝑦𝐼,
(9.22a)
LS-DYNA Theory Manual 
Belytschko-Lin-Tsay Shell 
𝑑 ̂
𝑦 = 𝐵2𝐼𝜐̂𝑦𝐼 − 𝑧̂𝐵2𝐼𝜃̂
𝑥𝐼,
2𝑑 ̂
𝑥𝑦 = 𝐵2𝐼 𝜐̂𝑥𝐼 + 𝐵1𝐼𝜐̂𝑦𝐼 + 𝑧̂ (𝐵2𝐼𝜃̂
𝑦𝐼 − 𝐵1𝐼𝜃̂
𝑥𝐼),
2𝑑 ̂
𝑥𝑧 = 𝐵1𝐼𝜐̂𝑧𝐼 + 𝑁𝐼𝜃̂
𝑦𝐼,
2 𝑑 ̂
𝑦𝑧 = 𝐵2𝐼 𝜐̂𝑧𝐼 − 𝑁𝐼 𝜃̂
𝑥𝐼,
𝐵1𝐼 =
𝐵2𝐼 =
∂𝑁𝐼
∂𝑥̂
,
∂𝑁𝐼
∂𝑦̂
.
(9.22b)
(9.22c)
(9.22d)
(9.22e)
(9.22f)
(9.22g)
The shape function derivatives 𝐵𝑎𝐼 are also evaluated at the center of the element, i.e., at 
𝜉 = 0, and 𝜂 = 0. 
9.3  Stress Resultants and Nodal Forces 
After  suitable  constitutive  evaluations  using  the  above  velocity-strains,  the 
resulting  stresses  are  integrated  through  the  thickness  of  the  shell  to  obtain  local 
resultant forces and moments.  The integration formula for the resultants are 
𝑓 ̂
𝑅 = ∫ 𝜎̂𝛼𝛽𝑑𝑧̂,
𝛼𝛽
𝑚̂𝛼𝛽
𝑅 = − ∫ 𝑧̂𝜎̂𝛼𝛽𝑑𝑧̂,
(9.23)
(9.24)
where  the  superscript,  𝑅,  indicates  a  resultant  force  or  moment,  and  the  Greek 
subscripts emphasize the limited range of the indices for plane stress plasticity. 
The above element-centered force and moment resultants are related to the local 
nodal  forces  and  moments  by  invoking  the  principle  of  virtual  power  and  integrating 
with a one-point quadrature.  The relations obtained in this manner are 
𝑅 + 𝐵2𝐼𝑓 ̂
𝑥𝐼 = 𝐴(𝐵1𝐼𝑓 ̂
𝑓 ̂
𝑅 ),
𝑥𝑦
𝑥𝑥
(9.25)
𝑅 + 𝐵1𝐼𝑓 ̂
𝑦𝐼 = 𝐴(𝐵2𝐼𝑓 ̂
𝑓 ̂
𝑅 ),
𝑥𝑦
𝑦𝑦
𝑅 + 𝐵2𝐼𝑓 ̂
𝑧𝐼 = 𝐴𝜅(𝐵1𝐼𝑓 ̂
𝑓 ̂
𝑅 ),
𝑦𝑧
𝑥𝑧
𝑚̂𝑥𝐼 = 𝐴 (𝐵2𝐼𝑚̂𝑦𝑦
𝑅 + 𝐵1𝐼𝑚̂𝑥𝑦
𝑅 −
𝑓 ̂
𝑅 ),
𝑦𝑧
𝑚̂𝑦𝐼 = −𝐴 (𝐵1𝐼𝑚̂𝑥𝑥
𝑅 + 𝐵2𝐼𝑚̂𝑥𝑦
𝑅 −
𝑓 ̂
𝑅 ),
𝑥𝑧
(9.26)
(9.27)
(9.28)
(9.29)
Belytschko-Lin-Tsay Shell 
LS-DYNA Theory Manual 
𝑚̂𝑧𝐼 = 0,
(9.30)
where 𝐴 is the area of the element, and 𝜅 is the shear factor from the Mindlin theory.  In 
the  Belytschko-Lin-Tsay  formulation,  𝜅  is  used  as  a  penalty  parameter  to  enforce  the 
Kirchhoff normality condition as the shell becomes thin. 
The  above  local  nodal  forces  and  moments  are  then  transformed  to  the  global 
coordinate system using the transformation relations given previously as Equation (9.8).  
The  global  nodal  forces  and  moments  are  then  appropriately  summed  over  all  the 
nodes  and  the  global  equations  of  motion  are  solved  for  the  next  increment  in  nodal 
accelerations. 
9.4  Hourglass Control (Belytschko-Lin-Tsay) 
In  part,  the  computational  efficiency  of  the  Belytschko-Lin-Tsay  and  the  under 
integrated  Hughes-Liu  shell  elements  are  derived  from  their  use  of  one-point 
quadrature in the plane of the element.  To suppress the hourglass deformation modes 
that  accompany  one-point  quadrature,  hourglass  viscosity  stresses  are  added  to  the 
physical stresses at the local element level.  The discussion of the hourglass control that 
follows pertains to the Hughes-Liu and the membrane elements as well. 
The hourglass control used by Belytschko et al., extends an earlier derivation by 
Flanagan  and  Belytschko  [1981],  .  The hourglass shape vector, 𝛕𝐼, is defined as 
𝛕𝐼 = 𝐡𝐼 − (𝐡𝐽𝐱̂𝑎𝐽)𝐁𝑎𝐼,
(9.31)
where 
+1
⎤
⎡
−1
⎥⎥
⎢⎢
, 
+1
−1⎦
⎣
is  the  basis  vector that  generates  the  deformation  mode that  is  neglected  by  one-point 
quadrature.  In Equation (9.31) and the reminder of this subsection, the Greek subscripts 
have a range of 2, e.g., 𝐱̂𝑎𝐼 = (𝑥̂1𝐼, 𝑥̂2𝐼) = (𝑥̂𝐼, 𝑦̂𝐼). 
𝐡 =
(9.32)
The hourglass shape vector then operates on the generalized displacements, in a 
manner  similar  to  Equations  (7.11a  -  e),  to  produce  the  generalized  hourglass  strain 
rates 
𝐵 = 𝛕𝐼𝜃̂
𝐪̇𝛼
𝛼𝐼,
𝐵 = 𝝉𝐼𝜐̂𝑧𝐼,
𝐪̇3
(9.33)
(9.34)
LS-DYNA Theory Manual 
Belytschko-Lin-Tsay Shell 
where  the  superscripts  𝐁  and  𝐌  denote  bending  and  membrane  modes,  respectively.  
The corresponding hourglass stress rates are then given by 
𝑀 = 𝛕𝐼𝜐̂𝛼𝐼,
𝐪̇𝛼
(9.35)
𝑄̇𝛼
𝐵 =
𝑟𝜃𝐸𝑡3𝐴
192
𝐵,
𝐵𝛽𝐼𝐵𝛽𝐼𝑞 ̇𝛼
𝑄̇3
𝐵 =
𝑟𝑤𝜅𝐺𝑡3𝐴
12
𝐵,
𝐵𝛽𝐼𝐵𝛽𝐼𝑞 ̇3
𝑄̇𝛼
𝑀 =
𝑟𝑚𝐸𝑡𝐴
𝐵𝛽𝐼𝐵𝛽𝐼𝑞 ̇𝛼
𝑀,
(9.36)
(9.37)
(9.38)
where 𝑡 is the shell thickness and the parameters, 𝑟𝜃, 𝑟𝑤, and 𝑟𝑚 are generally assigned 
values between 0.01 and 0.05. 
Finally,  the  hourglass  stresses,  which  are  updated  from  the  stress  rates  in  the 
usual way, i.e.,  
and the hourglass resultant forces are then 
𝐐𝑛+1 = 𝐐𝑛 + Δ𝑡𝐐̇ ,
𝑚̂𝛼𝐼
𝐵,
𝐻 = 𝜏𝐼𝑄𝛼
𝐵,
𝑓 ̂
𝐻 = 𝜏𝐼𝑄3
3𝐼
𝑓 ̂
𝑀,
𝐻 = 𝜏𝐼𝑄𝛼
𝛼𝐼
(9.39)
(9.40)
(9.41)
(9.42)
where the superscript 𝐻 emphasizes that these are internal force contributions from the 
hourglass  deformations.    These  hourglass  forces  are  added  directly  to  the  previously 
determined local internal forces due to deformations Equations (7.14a - f).  These force 
vectors are orthogonalized with respect to rigid body motion. 
9.5  Hourglass Control (Englemann and Whirley) 
Englemann  and  Whirley  [1991]  developed  an  alternative  hourglass  control, 
which  they  implemented  in  the  framework  of  the  Belytschko,  Lin,  and  Tsay  shell 
element.    We  will  briefly  highlight  their  procedure  here  that  has  proven  to  be  cost 
effective-only twenty percent more expensive than the default control. 
In the hourglass procedure, the in-plane strain field (subscript p) is decomposed 
into the one point strain field plus the stabilization strain field: 
𝑠 ,
0 + 𝛆̅
̇p
̇p
̇p = 𝛆̅
𝛆̅
(9.43)
Belytschko-Lin-Tsay Shell 
LS-DYNA Theory Manual 
𝑠 = 𝐖𝑚𝐪̇𝑚 + 𝑧𝐖𝑏𝐪̇𝑏.
̇p
𝛆̅
(9.44)
Here, 𝐖𝑚 and 𝐖𝑏 play the role of stabilization strain velocity operators for membrane 
and bending: 
𝐖𝑚 =
𝑝(𝜉 , 𝜂)
𝑓1
⎡
𝑝(𝜉 , 𝜂)
⎢
𝑓2
⎢
𝑝(𝜉 , 𝜂)
𝑓3
⎣
𝑝(𝜉 , 𝜂)
𝑓4
⎤
𝑝(𝜉 , 𝜂)
⎥
, 
𝑓5
⎥
𝑝(𝜉 , 𝜂)⎦
𝑓6
𝐖𝑏 =
−𝑓4
⎡
⎢
−𝑓5
⎢
−𝑓6
⎣
𝑝(𝜉 , 𝜂)
𝑝(𝜉 , 𝜂)
𝑝(𝜉 , 𝜂)
𝑝(𝜉 , 𝜂)
𝑓1
⎤
𝑝(𝜉 , 𝜂)
⎥
, 
𝑓2
⎥
𝑝(𝜉 , 𝜂)⎦
𝑓3
(9.45)
(9.46)
where the terms 𝑓𝑖
to the reference [Englemann and Whirley, 1991]. 
𝑝(𝜉 , 𝜂) 𝑖 = 1, 2, . . . , 6, are rather complicated and the reader is referred 
To  obtain  the  transverse  shear  assumed  strain  field,  the  procedure  given  in 
[Bathe  and  Dvorkin,  1984]  is  used.    The  transverse  shear  strain  field  can  again  be 
decomposed into the one point strain field plus the stabilization field: 
that is related to the hourglass velocities by 
𝑠,
0 + 𝛆̅
̇s
̇s
̇s = 𝛆̅
𝛆̅
𝑠 = 𝐖s𝐪̇𝑠,
̇s
𝛆̅
where the transverse shear stabilization strain-velocity operator 𝐖𝑠 is given by 
𝑠(𝜉 , 𝜂) −𝑔1
𝑠𝜉
𝑓1
𝑠𝜉
𝑠(𝜉 , 𝜂)
𝑔4
𝑓2
𝑠(𝜉 , 𝜂) and 𝑔1
𝑠𝜉
𝑠𝜂
𝑔2
𝑔3
𝑠𝜉
𝑠𝜂 −𝑔2
𝑔4
𝑠 are defined in the reference. 
Again, the coefficients 𝑓1
𝑠𝜂
𝑔3
𝑠𝜂
𝑔1
𝐖𝑠 = [
].
(9.47)
(9.48)
(9.49)
In  their  formulation,  the  hourglass  forces  are  related  to  the  hourglass  velocity 
field through an incremental hourglass constitutive equation derived from an additive 
decomposition of the stress into a “one-point stress,” plus a “stabilization stress.”  The 
integration  of  the  stabilization  stress  gives  a  resultant  constitutive  equation  relating 
hourglass  forces  to  hourglass  velocities.    The  in-plane  and  transverse  stabilization 
stresses are updated according to: 
𝑠,𝑛+1 = 𝛕s
𝛕s
𝑠,
𝑠,𝑛 + Δ𝑡𝑐𝑠𝐂𝑠𝛆̅
̇𝑠
(9.50)
𝑠,
𝑠,𝑛 + Δ𝑡𝑐s𝐂s𝛆̅
̇s
where the tangent matrix is the product of a matrix 𝐂, which is constant within the shell 
domain, and a scalar 𝑐 that is constant in the plane but may vary through the thickness. 
𝑠,𝑛+1 = 𝛕s
𝛕s
(9.51)
The stabilization stresses can now be used to obtain the hourglass forces:
LS-DYNA Theory Manual 
Belytschko-Lin-Tsay Shell 
Figure  9.2.    The  twisted  beam  problem  fails  with  the  Belytschko-Tsay  shell 
element. 
𝐐𝑚 = ∫ ∫ 𝐖𝑚
−ℎ
T 𝛕𝑝
𝑠 𝑑𝐴
,
𝑑𝑧
𝐐𝑏 = ∫ ∫ 𝐖𝑏
−ℎ
T𝛕𝑝
𝑠 𝑑𝐴
𝐐𝑠 = ∫ ∫ 𝐖𝑠
−ℎ
T𝛕𝑠
𝑠𝑑𝐴
𝑑𝑧
,
𝑑𝑧
.
(9.52)
(9.53)
(9.54)
9.6  Belytschko-Wong-Chiang Improvements 
Since the Belytschko-Tsay element is based on a perfectly flat geometry, warpage 
is not considered.  Although this generally poses no major difficulties and provides for 
an  efficient  element,  incorrect results  in  the  twisted  beam  problem,  See  Figure  7.2,  are 
obtained  where  the  nodal  points  of  the  elements  used  in  the  discretization  are  not 
coplanar.    The  Hughes-Liu  shell  element  considers  non-planar  geometry  and  gives 
good results on the twisted beam, but is relatively expensive.  The effect of neglecting 
warpage in typical a application cannot be predicted beforehand and may lead to less 
than  accurate  results,  but  the  latter  is  only  speculation  and  is  difficult  to  verify  in 
practice.  Obviously, it would be better to use shells that consider warpage if the added 
costs are reasonable and if this unknown effect is eliminated.  In this section we briefly 
describe  the  simple  and  computationally  inexpensive  modifications  necessary  in  the 
Belytschko-Tsay shell to include the warping stiffness.  The improved transverse shear 
treatment  is  also  described  which  is  necessary  for  the  element  to  pass  the  Kirchhoff
Belytschko-Lin-Tsay Shell 
LS-DYNA Theory Manual 
P3
P1
P2
Figure 9.3.  Nodal fiber vectors 𝐩1, 𝐩2, and 𝐩3, where ℎ is the thickness. 
patch test.  Readers are directed to the references [Belytschko, Wong, and Chang 1989, 
1992] for an in depth theoretical background. 
In  order  to  include  warpage  in  the  formulation  it  is  convenient  to  define  nodal 
fiber vectors  as  shown  in  Figure  7.3.    The  geometry  is  interpolated  over the  surface  of 
the shell from: 
where 
𝑥 = 𝑥𝑚 + 𝜁 ̅𝑝 = (𝑥𝐼 + 𝜁 ̅𝑝𝐼)𝑁𝐼(𝜉 , 𝜂),
𝜁 ̅ =
𝜁ℎ
.
The in plane strain components are given by: 
𝑑𝑥𝑥 = 𝑏𝑥𝐼𝑣̂𝑥𝐼 + 𝜁 ̅(𝑏𝑥𝐼
𝑐 𝑣̂𝑥𝐼 + 𝑏𝑥𝐼𝑝̇𝑥𝐼),
𝑑𝑦𝑦 = 𝑏𝑦𝐼𝑣̂𝑦𝐼 + 𝜁 ̅(𝑏𝑦𝐼
𝑐 𝑣̂𝑦𝐼 + 𝑏𝑦𝐼𝑝̇𝑦𝐼),
𝑑𝑥𝑦 =
𝑏𝑥𝐼𝑣̂𝑦𝐼 + 𝑏𝑦𝐼𝑣̂𝑥𝐼 + 𝜁 ̅(𝑏𝑥𝐼
𝑐 𝑣̂𝑦𝐼 + 𝑏𝑥𝐼𝑝̇𝑦𝐼 + 𝑏𝑦𝐼
𝑐 𝑣̂𝑥𝐼 + 𝑏𝑦𝐼𝑝̇𝑥𝐼). 
(9.55)
(9.56)
(9.57)
(9.58)
(9.59)
The  coupling  terms  are  come  in  through  𝑏𝑖𝐼
components of the fiber vectors as: 
𝑐 :  which  is  defined  in  terms  of  the 
𝑏𝑥𝐼
𝑐 } = [
𝑏𝑦𝐼
{
𝑝𝑦̂2 − 𝑝𝑦̂4
𝑝𝑥̂2 − 𝑝𝑥̂4
𝑝𝑦̂3 − 𝑝𝑦̂1
𝑝𝑥̂3 − 𝑝𝑥̂1
𝑝𝑦̂4 − 𝑝𝑦̂2
𝑝𝑥̂4 − 𝑝𝑥̂2
𝑝𝑦̂1 − 𝑝𝑦̂3
𝑝𝑥̂1 − 𝑝𝑥̂3
], 
(9.60)
For a flat geometry the normal vectors are identical and no  coupling can occur.  
𝑐  and the reader is referred to his 
Two methods are used by Belytschko for computing 𝑏𝑖𝐼
papers  for  the  details.    Both  methods  have  been  tested  in  LS-DYNA  and  comparable 
results were obtained. 
The transverse shear strain components are given as
LS-DYNA Theory Manual 
Belytschko-Lin-Tsay Shell 
y^
ey^
Lk
enk
eni
ex^
Figure  9.4.    Vector  and  edge  definitions  for  computing  the  transverse  shear
strain components. 
𝛾̂𝑥𝑧 = −𝑁𝐼(𝜉 , 𝜂)𝜃̅
𝑦̂𝐼,
𝛾̂𝑦𝑧 = −𝑁𝐼(𝜉 , 𝜂)𝜃̅
𝑥̂𝐼,
where the nodal rotational components are defined as: 
𝐾,
𝐾 ⋅ 𝐞𝑥̂)𝜃̅
𝐼 + (𝐞𝑛
𝐼 ⋅ 𝐞𝑥̂)𝜃̅
𝜃̅
𝑥̂𝐼 = (𝐞𝑛
𝜃̅
𝑦̂𝐼 = (𝐞𝑛
𝐼 + (𝐞𝑛
𝐼 ⋅ 𝐞𝑦̂)𝜃̅
𝐾,
𝐾 ⋅ 𝐞𝑦̂)𝜃̅
𝐼 =
𝜃̅
(𝜃𝑛𝐼
𝐼 + 𝜃𝑛𝐽
𝐼 ) +
𝐿𝐼𝐽 (𝜐̂𝑧𝐽 − 𝜐̂𝑧𝐽),
(9.61)
(9.62)
(9.63)
(9.64)
(9.65)
where the subscript n refers to the normal component of side 𝐼 as seen in Figure 7.3 and 
𝐿𝐼𝐽 is the length of side 𝐼𝐽.
LS-DYNA Theory Manual 
Triangular Shells 
10    
Triangular Shells 
10.1  C0 Triangular Shell 
The  𝐶0  shell  element  due  to  Kennedy,  Belytschko,  and  Lin  [1986]  has  been 
implemented  as  a  computationally  efficient  triangular  element  complement  to  the 
Belytschko-Lin-Tsay  quadrilateral  shell  element 
([Belytschko  and  Tsay  1981], 
[Belytschko  et  al.,  1984a]).    For  a  shell  element  with  five  through-the-thickness 
integration  points,  the  element  requires  649  mathematical  operations  (the  Belytschko-
Lin-Tsay quadrilateral shell element requires 725 mathematical operations) compared to 
1417  operations  for  the  Marchertas-Belytschko  triangular  shell  [Marchertas  and 
Belytschko  1974]  (referred  to  as  the  BCIZ  [Bazeley,  Cheung,  Irons,  and  Zienkiewicz 
1965] triangular shell element in the DYNA3D user’s manual). 
Triangular  shell  elements  are  offered  as  optional  elements  primarily  for 
compatibility with local user grid generation and refinement software.  Many computer 
aided design (CAD) and computer aided manufacturing (CAM) packages include finite 
element mesh generators, and most of these mesh generators use triangular elements in 
the discretization.  Similarly, automatic mesh refinement algorithms are typically based 
on triangular element discretization.  Also, triangular shell element formulations are not 
subject to zero energy modes inherent in quadrilateral element formulations. 
The triangular shell element’s origins are based on the work of Belytschko et al., 
[Belytschko, Stolarski, and Carpenter 1984b] where the linear performance of the  shell 
was demonstrated.  Because the triangular shell element formulations parallels closely 
the formulation of the Belytschko-Lin-Tsay quadrilateral shell element presented in the 
previous  section  (Section  7),  the  following  discussion  is  limited  to  items  related 
specifically to the triangular shell element. 
10.1.1  Co-rotational Coordinates 
The  mid-surface  of  the  triangular  shell  element,  or  reference  surface,  is  defined 
by the location of the element’s three nodes.  An embedded element coordinate system
Triangular Shells 
LS-DYNA Theory Manual 
y^
z^
e^
e^
e^
x^
Figure 10.1.  Local element coordinate system for C0 shell element. 
  that  deforms  with  the  element  is  defined  in  terms  of  these  nodal 
coordinates.    The  procedure  for  constructing  the  co-rotational  coordinate  system  is 
simpler than the corresponding procedure for the quadrilateral, because the three nodes 
of the triangular element are guaranteed coplanar. 
The  local  x-axis  𝑥̂  is  directed  from  node  1  to  2.    The  element’s  normal  axis  𝑧̂  is 
defined by the vector cross product of a vector along 𝑥̂ with a vector constructed from 
node 1 to node 3.  The local y-axis 𝑦̂ is defined by a unit vector cross product of  𝐞̂3 with 
𝐞̂1,  which  are  the  unit  vectors  in  the  𝑧̂  directions,  respectively.    As  in  the  case  of  the 
quadrilateral  element,  this  triad  of  co-rotational  unit  vectors  defines  a  transformation 
between the global and local element coordinate systems.  See Equations (7.5 a, b). 
10.1.2  Velocity-Strain Relations 
As  in  the  Belytschko-Lin-Tsay  quadrilateral  shell  element,  the  displacement  of 
any point in the shell is partitioned into a mid-surface displacement (nodal translations) 
and  a  displacement  associated  with  rotations  of  the  element’s  fibers  (nodal  rotations).  
The  Kennedy-Belytschko-Lin  triangular  shell  element  also  uses  the  Mindlin  [Mindlin 
1951] theory of plates and shells to partition the velocity of any point in the shell (recall 
Equation (7.6)): 
𝐯 = 𝐯m − 𝑧̂ 𝐞3 × 𝛉,
(10.1)
where 𝐯m is the velocity of the mid-surface, 𝛉 is the angular velocity vector, and 𝑧̂ is the 
distance  along  the  fiber  direction  (thickness)  of  the  shell  element.    The  corresponding 
co-rotational  components  of  the  velocity  strain  (rate  of  deformation)  were  given 
previously in Equation (7.11 a - e). 
Standard  linear  nodal  interpolation  is  used  to  define  the  midsurface  velocity, 
angular  velocity,  and  the  element’s  coordinates  (isoparametric  representation).    These 
interpolation 
triangular  element 
formulations.  Substitution of the nodally interpolated velocity fields into the velocity-
strain relations , leads to strain rate-velocity relations of 
the form 
the  area  coordinates  used 
functions  are 
in 
10-2 (Triangular Shells) 
𝐝̂ = 𝐁 𝐯̂.
LS-DYNA Theory Manual 
Triangular Shells 
It is convenient to partition the velocity strains and the 𝐁 matrix into membrane 
and bending contributions.  The membrane relations are given by 
⎧ 𝑑 ̂
{{
𝑑 ̂
⎨
{{
2𝑑 ̂
⎩
⎫
}}
⎬
}}
𝑥𝑦⎭
=
𝑦̂3
⎡
⎢
𝑥̂2𝑦̂3 ⎣
𝑥̂3 − 𝑥̂2
𝑥̂3 − 𝑥̂2
−𝑦̂3
𝑦̂3
−𝑥̂3
−𝑥̂3
𝑦̂3
𝑥̂2
⎤
𝑥̂2
⎥
0 ⎦
⎫
⎧𝜐̂𝑥1
𝜐̂𝑦1
𝜐̂𝑥2
𝜐̂𝑦2
𝜐̂𝑥3
𝜐̂𝑦3⎭
{{{{{
{{{{{
}}}}}
}}}}}
⎬
⎨
⎩
, 
(10.3)
𝐝̂M = 𝐁M 𝐯̂,
(10.4)
⎧ 𝜅̂𝑥
⎫
}
{
𝜅̂𝑦
⎬
⎨
}
{
2𝜅̂𝑥𝑦⎭
⎩
=
−1
⎡
𝑥̂3 − 𝑥̂2
⎢
𝑥̂2𝑦̂3 ⎣
𝑦̂3
or 
−𝑦̂3
𝑦̂3
𝑥̂3 − 𝑥̂2 −𝑦̂3 −𝑥̂3
𝑥̂3
−𝑥̂2
⎤
⎥
𝑥̂2⎦
⎫
⎧𝜃̂
𝑥1
𝜃̂
𝑦1
𝜃̂
𝑥2
⎨
𝜃̂
𝑦2
𝜃̂
𝑥3
𝜃̂
𝑦3⎭
⎩
{{{{{{
{{{{{{
}}}}}}
}}}}}}
⎬
, 
(10.5)
𝛋̂M = 𝐁M𝛉̂ def.
(10.6)
The local element velocity strains are then obtained by combining the above two 
relations: 
⎧ 𝑑 ̂
{{
𝑑 ̂
⎨
{{
2𝑑 ̂
⎩
⎫
}}
⎬
}}
𝑥𝑦⎭
=
⎧ 𝑑 ̂
{{
𝑑 ̂
⎨
{{
2𝑑 ̂
⎩
⎫
}}
⎬
}}
𝑥𝑦⎭
− 𝑧̂ 
⎧ 𝜅̂𝑥
⎫
}
{
𝜅̂𝑦
⎬
⎨
}
{
2𝜅̂𝑥𝑦⎭
⎩
= 𝐝̂M − 𝑧̂𝛋̂. 
(10.7)
The remaining two transverse shear strain rates are given by 
{
6 𝑥̂2 𝑦̂3
} =
2𝑑 ̂
𝑥𝑧
2𝑑 ̂
𝑦𝑧
−𝑦̂3
[
𝑦̂3( 𝑥̂2 − 2𝑥̂2)
𝑦̂3 (2 𝑥̂2 + 𝑥̂3) 𝑦̂3
2 − 𝑥̂3
𝑥̂2
−𝑦̂3
𝑦̂3(3 𝑥̂2 − 𝑥̂3)
2( 𝑥̂2 + 𝑥̂3) 𝑥̂3( 𝑥̂3 − 2𝑥̂2) −3𝑥̂2𝑦̂3
(10.8)
𝑥̂2𝑦̂3
]
𝑥̂2( 2𝑥̂3 − 𝑥̂2)
Triangular Shells 
LS-DYNA Theory Manual 
def
, 
⎫
⎧𝜃̂
𝑥1
𝜃̂
𝑦1
𝜃̂
𝑥2
𝜃̂
𝑦2
𝜃̂
𝑥3
𝜃̂
𝑦3⎭
{{{{{{
{{{{{{
}}}}}}
}}}}}}
⎨
⎩
⎬
All  of  the  above  velocity-strain  relations  have  been  simplified  by  using  one-point 
quadrature. 
𝐝̂S = 𝐁S𝛉̂ def.
(10.9)
In the above relations, the angular velocities 𝛉̂def are the deformation component 
of the angular velocity 𝛉̂ obtained by subtracting the portion of the angular velocity due 
to rigid body rotation, i.e., 
The two components of the rigid body angular velocity are given by 
𝛉̂def = 𝛉̂ − 𝛉̂rig,
rig =
𝜃̂
𝜐̂𝑧1 − 𝜐̂𝑧2
𝑥̂2
,
(10.10)
(10.11)
rig =
𝜃̂
(𝜐̂𝑧3 − 𝜐̂𝑧1)𝑥̂2 − (𝜐̂𝑧2 − 𝜐̂𝑧1)𝑥̂3
𝑥̂2𝑦̂3
The  first  of  the  above  two  relations  is  obtained  by  considering  the  angular  velocity  of 
the local x-axis about the local y-axis.  Referring to Figure 10.1, by construction nodes 1 
and 2 lie on the local x-axis and the distance between the nodes is 𝑥̂2 i.e., the 𝑥̂ distance 
from node 2 to the local coordinate origin at node 1.  Thus the difference in the nodal 𝑧̂ 
velocities divided by the distance between the nodes is an average measure of the rigid 
body rotation rate about the local y-axis. 
(10.12)
.
The  second  relation  is  conceptually  identical,  but  is  implemented  in  a  slightly 
different manner due to the arbitrary location of node 3 in the local coordinate system.  
Consider  the  two  local  element  configurations  shown  in  Figure  10.2.    For  the  leftmost 
configuration,  where  node  3  is  the  local  y-axis,  the  rigid  body  rotation  rate  about  the 
local x-axis is given by 
rig =
𝜃̂
𝑥−left
𝜐̂𝑧3 − 𝜐̂𝑧1
𝑦̂3
,
and for the rightmost configuration the same rotation rate is given by 
rig
𝜃̂
𝑥−right
=
𝜐̂𝑧3 − 𝜐̂𝑧2
𝑦̂3
.
(10.13)
(10.14)
LS-DYNA Theory Manual 
Triangular Shells 
z^
y^
z^
x^
y^
x^
Figure  10.2.    Element  configurations  with  node  3  aligned  with  node  1  (left) 
and node 3 aligned with node 2 (right). 
Although both of these relations yield the average rigid body rotation rate, the selection 
of the correct relation depends on the configuration of the element, i.e., on the location 
of node 3.  Since every element in the mesh could have a configuration that is different 
in  general  from  either  of  the  two  configurations  shown  in  Figure  10.2,  a  more  robust 
relation  is  needed  to determine  the  average  rigid  body  rotation  rate  about  the  local  x-
axis.    In  most  typical  grids,  node  3  will  be  located  somewhere  between  the  two 
configurations  shown  in  Figure  10.2.    Thus  a  linear  interpolation  between  these  two 
rigid body rotation rates was devised using the distance 𝑥̂3 as the interpolant: 
rig = 𝜃̂
𝜃̂
rig (1 −
𝑥−left
𝑥̂3
𝑥̂2
) + 𝜃̂
rig
𝑥−right
(
𝑥̂3
𝑥̂2
).
(10.15)
Substitution  of Equations  (10.13)  and  (10.14)  into (10.15)  and  simplifying  produces  the 
relations given previously as Equation (10.12).
Triangular Shells 
LS-DYNA Theory Manual 
10.1.3  Stress Resultants and Nodal Forces 
After  suitable  constitutive  evaluation  using  the  above  velocity  strains,  the 
resulting  local  stresses  are  integrated  through  the  thickness  of  the  shell  to  obtain  local 
resultant forces and moments.  The integration formulae for the resultants are 
𝑓 ̂
𝑅 = ∫ 𝜎̂𝛼𝛽𝑑𝑧̂,
𝛼𝛽
𝑚̂𝛼𝛽
𝑅 = − ∫ 𝑧̂ 𝜎̂𝛼𝛽𝑑𝑧̂,
(10.16)
(10.17)
where the superscript 𝑅 indicates a resultant force or moment and the Greek subscripts 
emphasize the limited range of the indices for plane stress plasticity. 
The above element-centered force and moment resultant are related to the local 
nodal forces and moments by invoking the principle of virtual power and performing a 
one-point quadrature.  The relations obtained in this manner are 
⎧𝑓 ̂
⎫
𝑥1
}
{
}
{
𝑓 ̂
}
{
𝑦1
}
{
}
{
𝑓 ̂
}
{
𝑥2
⎬
⎨
𝑓 ̂
}
{
𝑦2
}
{
}
{
𝑓 ̂
}
{
𝑥3
}
{
}
{
𝑓 ̂
⎩
𝑦3⎭
= 𝐴𝐁M
⎧𝑓 ̂
𝑥𝑥
{{
𝑓 ̂
⎨
𝑦𝑦
{{
𝑓 ̂
⎩
𝑥𝑦
⎫
}}
⎬
}}
⎭
, 
= 𝐴𝐁M
⎧𝑚̂𝑥𝑥
{{
𝑚̂𝑦𝑦
⎨
{{
𝑚̂𝑥𝑦
⎩
⎫
}}
⎬
}}
⎭
+ 𝐴𝐁S
T  {
𝑓 ̂
 𝑅
𝑥𝑧
 𝑅}, 
𝑓 ̂
𝑦𝑧
(10.18)
(10.19)
⎫
⎧𝑚̂𝑥1
𝑚̂𝑦1
𝑚̂𝑥2
𝑚̂𝑦2
𝑚̂𝑥3
𝑚̂𝑦3⎭
{{{{{
{{{{{
}}}}}
}}}}}
⎬
⎨
⎩
where 𝐴 is the area of the element (2𝐴 = 𝑥̂2𝑦̂3). 
The  remaining  nodal  forces,  the  𝑧̂  component  of  the  force  (𝑓 ̂
determined by successively solving the following equilibration equations 
𝑚̂𝑥1 + 𝑚̂𝑥2 + 𝑚̂𝑥3 + 𝑦̂3𝑓 ̂
𝑧3 = 0,
𝑧3 , 𝑓 ̂
𝑧2 , 𝑓 ̂
𝑧1),  are 
𝑚̂𝑦1 + 𝑚̂𝑦2 + 𝑚̂𝑦3 − 𝑥̂3𝑓 ̂
𝑧3 − 𝑥̂2𝑓 ̂
𝑧2 = 0,
𝑧1 + 𝑓 ̂
𝑓 ̂
𝑧2 + 𝑓 ̂
𝑧3 = 0,
(10.20)
(10.21)
(10.22)
which represent moment equilibrium about the local x-axis, moment equilibrium about 
the local y-axis, and force equilibrium in the local z-direction, respectively.
LS-DYNA Theory Manual 
Triangular Shells 
10.2  Marchertas-Belytschko Triangular Shell 
The  Marchertas-Belytschko  [1974]  triangular  shell  element,  or  the  BCIZ 
triangular  shell  element  as  it  is  referred  to  in  the  LS-DYNA  user’s  manual,  was 
developed  in  the  same  time  period  as  the  Belytschko  beam  element  [Belytschko, 
Schwer,  and  Klein,  1977],  see  Section  4,  forming  the  first  generation  of  co-rotational 
structural  elements  developed  by  Belytschko  and  co-workers.    This  triangular  shell 
element  became  the  first  triangular  shell  implemented  in  DYNA3D.    Although  the 
Marchertas-Belytschko shell element is relatively expensive, i.e., the 𝐶0 triangular shell 
element  with  five  through-the-thickness  integration  points  requires  649  mathematical 
operations compared to 1,417 operations for the Marchertas-Belytschko triangular shell, 
it  is  maintained  in  LS-DYNA  for  compatibility  with  earlier  user  models.    However,  as 
the LS-DYNA user community moves to application of the more efficient shell element 
formulations,  the  use  of  the  Marchertas-Belytschko  triangular  shell  element  will 
decrease. 
As  mentioned  above,  the  Marchertas-Belytschko  triangular  shell  has  a  common 
co-rotational  formulation  origin  with  the  Belytschko  beam  element.    The  interested 
reader is referred to the beam element description, see Section 4, for details on the co-
rotational  formulation.    In  the  next  subsection  a  discussion  of  how  the  local  element 
coordinate  system  is  identical  for  the  triangular  shell  and  beam  elements.    The 
remaining  subsections  discuss  the  triangular  element’s  displacement  interpolants,  the 
strain displacement relations, and calculations of the element nodal forces.  In the report 
[1974], much greater detail is provided. 
10.2.1  Element Coordinates 
Figure 10.3(a) shows the element coordinate system, (𝐱̂, 𝐲̂, 𝐳̂) originating at Node 
1,  for  the  Marchertas-Belytschko  triangular  shell.    The  element  coordinate  system  is 
associated  with  a  triad  of  unit  vectors  (𝐞1, 𝐞2, 𝐞3)  the  components  of  which  form  a 
transformation  matrix  between  the  global  and  local  coordinate  systems  for  vector 
quantities.  The nodal or body coordinate system unit vectors (𝐛1, 𝐛2, 𝐛3) are defined 
at  each  node  and  are  used  to  define  the  rotational  deformations  in  the  element,  see 
Section 8.4.4. 
The unit normal to the shell element 𝐞3 is formed from the vector cross product 
𝐞3 = 𝐥21 × 𝐥31,
(10.23)
where 𝐥21 and 𝐥31 are unit vectors originating at Node 1 and pointing towards Nodes 2 
and 3 respectively, see Figure 10.3(b). 
Next  a  unit  vector  g,  see  Figure  10.3(b),  is  assumed  to  be  in  the  plane  of  the 
triangular  element  with  its  origin  at  Node  1 and  forming  an  angle 𝛽  with  the  element 
side between Nodes 1 and 2, i.e., the vector 𝑙21.  The direction cosines of this unit vector
Triangular Shells 
LS-DYNA Theory Manual 
are  represented  by  the  symbols  (𝑔𝑥, 𝑔𝑦, 𝑔𝑧).    Since  g  is  the  unit  vector,  its  direction 
cosines will satisfy the equation 
𝑔𝑥
2 + 𝑔𝑦
2 + 𝑔𝑧
2 = 1.
(10.24)
Also,  since  𝐠  and  𝐞3  are  orthogonal  unit  vectors,  their  vector  dot  product  must 
satisfy the equation 
𝑒3𝑥𝑔𝑥 + 𝑒3𝑦𝑔𝑦 + 𝑒3𝑧𝑔𝑧 = 0.
(10.25)
In  addition,  the  vector  dot  product of  the  co-planar  unit  vectors 𝐠  and  𝐥21  satisfies  the 
equation 
𝐼21𝑥𝑔𝑥 + 𝐼21𝑦𝑔𝑦𝑔𝑦 + 𝐼21𝑧𝑔𝑧 = cos𝛽,
(10.26)
where (𝑙21𝑥, 𝑙21𝑦, 𝑙21𝑧)are the direction cosines of 𝐥21.
LS-DYNA Theory Manual 
Triangular Shells 
y^
z^
e2
e3
e1
x^
b2
(a) Element and body coordinates 
b3
b1
y^
z^
e2
I31
e3
α/2
I21
x^
b2
b3
b1
(b) Construction of element coordinates
Figure 10.3.  Construction of local element coordinate system. 
Solving this system of three simultaneous equation, i.e., Equation (10.24), (10.25), 
and (10.26), for the direction cosines of the unit vector g yields 
𝑔𝑥 = 𝑙21𝑥cos𝛽 + (𝑒3𝑦𝑙21𝑧 − 𝑒3𝑧𝑙21𝑦)sin𝛽,
𝑔𝑦 = 𝑙21𝑦cos𝛽 + (𝑒3𝑧𝑙21𝑥 − 𝑒3𝑥𝑙21𝑧)sin𝛽,
(10.27)
(10.28)
Triangular Shells 
LS-DYNA Theory Manual 
𝑔𝑧 = 𝑙21𝑧cos𝛽 + (𝑒3𝑥𝑙21𝑦 − 𝑒3𝑦𝑙21𝑥)sin𝛽.
(10.29)
These  equations  provide  the  direction  cosines  for  any  vector  in  the  plane  of  the 
triangular element that is oriented at an angle 𝛽 from the element side between Nodes 1 
and  2.    Thus  the  unit  vector  components  of  𝐞1  and  𝐞2  are  obtained  by  setting  𝛽 = 𝛼/2 
and  𝛽 = (𝜋 + 𝛼)/2  in  Equation  (8.22),  respectively.    The  angle  𝛼  is  obtained  from  the 
vector dot product of the unit vectors 𝐥21 and 𝐥31, 
cos𝛼 = 𝐥21 ⋅ 𝐥31.
(10.30)
10.2.2  Displacement Interpolation 
As  with  the  other  large  displacement  and  small  deformation  co-rotational 
element  formulations,  the  nodal  displacements  are  separated  into  rigid  body  and 
deformation displacements, 
𝐮 = 𝐮rigid + 𝐮def,
(10.31)
where  the  rigid  body  displacements  are  defined  by  the  motion  of  the  local  element 
coordinate system, i.e., the co-rotational coordinates, and the deformation displacement 
are  defined  with  respect  to  the  co-rotational  coordinates. 
  The  deformation 
displacement are defined by 
def
⎧ 𝑢̂𝑥
{{
𝑢̂𝑦
⎨
− − −
{{
⎩
⎫
}}
⎬
}}
𝑢̂𝑧 ⎭
=
𝜙𝑥
𝜙𝑦
− − −
𝜙𝑧
⎡
⎢
⎢
⎢
⎣
⎤
⎥
⎥
⎥
⎦
{⎧ 𝛿
}⎫
− − −
𝜃̂ ⎭}⎬
⎩{⎨
, 
𝛅T = {𝛿12
𝛿23
𝛿31},
are the edge elongations and 
𝛉̂ = {𝜃̂
1𝑥
𝜃̂
1𝑦
𝜃̂
2𝑥
𝜃̂
2𝑦
𝜃̂
3𝑥
𝜃̂
3𝑦},
are the local nodal rotation with respect to the co-rotational coordinates. 
(10.32)
(10.33)
(10.34)
𝑚,  𝜙𝑦
𝑚  and  𝜙𝑧
The  matrices  𝜙𝑥
𝑓   are  the  membrane  and  flexural  interpolation 
functions, respectively.  The element’s membrane deformation is defined in terms of the 
edge  elongations.    Marchertas  and  Belytschko  adapted  this  idea  from  Argyris  et  al., 
[1964], where incremental displacements are used, by modifying the relations for total 
displacements, 
𝛿𝑖𝑗 =
2(𝑥𝑗𝑖𝑢𝑗𝑖𝑥 + 𝑦𝑗𝑖𝑢𝑗𝑖𝑦 + 𝑧𝑗𝑖𝑢𝑗𝑖𝑧) + 𝑢𝑗𝑖𝑥
2 + 𝑢𝑗𝑖𝑦
2 + 𝑢𝑗𝑖𝑧
0 + 𝑙𝑖𝑗
𝑙 𝑖𝑗
, 
(10.35)
where 𝑥𝑗𝑖 = 𝑥𝑗 − 𝑥𝑖, etc. 
The  non-conforming  shape  functions  used  for  interpolating  the  flexural 
𝑓   were  originally  derived  by  Bazeley,  Cheung,  Irons,  and  Zienkiewicz 
deformations,  𝜙𝑧
LS-DYNA Theory Manual 
Triangular Shells 
𝑓  
[1965]; hence the LS-DYNA reference to the BCIZ element.  Explicit expressions for 𝜙𝑧
are quite tedious and are not given here.  The interested reader is referred to Appendix 
G in the original work of Marchertas and Belytschko [1974]. 
The  local  nodal  rotations,  which  are  interpolated  by  these  flexural  shape 
functions,  are  defined  in  a  manner  similar  to  those  used  in  the  Belytschko  beam 
element.  The current components of the original element normal are obtained from the 
relation 
0,
0 = 𝛍T𝛌𝐞̅ 3
𝐞3
(10.36)
where  𝛍  and  𝛌  are  the  current  transformations  between  the  global  coordinate  system 
 0 is the 
and the element (local) and body coordinate system, respectively.  The vector 𝐞̅ 3
original element unit normal expressed in the body coordinate system.  The vector cross 
product between this current-original unit normal and the current unit normal, 
𝐞3 × 𝐞3
0 = 𝜃̂
𝑥𝐞1 + 𝜃̂
𝑦𝐞2,
define the local nodal rotations as 
0 ,
𝛉̂𝑥 = − 𝐞̂3𝑦
0 .
𝛉̂𝑦 = 𝐞̂3𝑥
(10.37)
(10.38)
(10.39)
Note that at each node the corresponding 𝛌 transformation matrix is used in Equation 
(10.36). 
10.2.3  Strain-Displacement Relations 
Marchertas-Belytschko  impose  the  usual  Kirchhoff  assumptions  that  normals  to 
the midplane of the element remain straight and normal, to obtain 
𝑒𝑥𝑥 =
𝑒𝑦𝑦 =
∂𝑢𝑥
∂𝑥
∂𝑢𝑦
∂𝑦
− 𝑧
− 𝑧
∂2𝑢𝑧
∂𝑥2 ,
∂2𝑢𝑧
∂𝑦2 ,
2𝑒𝑥𝑦 =
∂𝑢𝑥
∂𝑦
+
∂𝑢𝑦
∂𝑥
− 2𝑧
∂2𝑢𝑧
∂𝑥 ∂𝑦
,
(10.40)
(10.41)
(10.42)
where it is understood that all quantities refer to the local element coordinate system. 
Substitution  of  Equations  (10.32)  into  the  above  strain-displacement  relations 
yields 
where 
𝛆 = 𝐄m𝜹 − 𝑧𝐄f𝛉̂,
T = {𝜀𝑥𝑥
𝛆   
𝜀𝑦𝑦
2𝜀𝑥𝑦},
(10.43)
(10.44)
Triangular Shells 
LS-DYNA Theory Manual 
with 
and 
𝐄m =
∂𝜙𝑥𝑖
∂𝑥
∂𝜙𝑦𝑖
∂𝑦
+
⎡
⎢
⎢
⎢
⎢
⎢
⎢
∂𝜙𝑥𝑖
⎢
∂𝑦
⎣
⎤
⎥
⎥
⎥
, 
⎥
⎥
⎥
∂𝜙𝑦𝑖
⎥
∂𝑥 ⎦
𝐄f =
⎡ ∂2𝜙𝑧𝑖
⎤
⎥
⎢
∂𝑥2
⎥
⎢
∂2𝜙𝑧𝑖
⎥
⎢
⎥
⎢
. 
⎥
⎢
∂𝑦2
⎥
⎢
⎥
⎢
∂2𝜙𝑧𝑖
⎥
⎢
∂𝑥 ∂𝑦⎦
⎣
(10.45)
(10.46)
Again, the interested reader is referred to Appendices F and G in the original work of 
Marchertas and Belytschko [1974] for explicit expressions of the above two matrices. 
10.2.4  Nodal Force Calculations 
The local element forces and moments are found by integrating the local element 
stresses through the thickness of the element.  The local nodal forces are given by 
𝐟 ̂ = ∫ 𝐄mT𝛔̂ 𝑑𝑉,
𝐟 ̂T = {𝑓12, 𝑓23, 𝑓31},
𝛔̂T = {𝜎𝑥𝑥, 𝜎𝑦𝑦, 𝜎𝑥𝑦},
(10.47)
(10.48)
(10.49)
where  the  side  forces  and  stresses  are  understood  to  all  be  in  the  local  convected 
coordinate system. 
Similarly, the local moments are given by 
𝐦̂ = − ∫ 𝑧 𝐄fT
𝛔̂ 𝑑𝑉,
 𝐦̂T = {𝑚̂1𝑥 𝑚̂1𝑦 𝑚̂2𝑥 𝑚̂2𝑦 𝑚̂3𝑥 𝑚̂3𝑦}.
(10.50)
(10.51)
The  through-the-thickness  integration  portions  of  the  above  local  force  and  moment 
integrals  are  usually  performed  with  a  3-  or  5-point  trapezoidal  integration.    A  three-
point  inplane  integration  is  also  used;  it  is  inpart  this  three-point  inplane  integration 
that  increases  the  operation  count  for  this  element  over  the 𝐶0  shell,  which  used  one-
point inplane integration with hourglass stabilization.
LS-DYNA Theory Manual 
Triangular Shells 
The  remaining  transverse  nodal  forces  are  obtained  from  element  equilibrium 
considerations.  Moment equilibrium requires 
{
𝑓 ̂
2𝑧
𝑓 ̂
3𝑧
} =
2𝐴
[
−𝑥̂3
𝑦̂3
 𝑥̂2 − 𝑦̂2
] {
𝑚̂1𝑥 + 𝑚̂2𝑥 + 𝑚̂3𝑥
𝑚̂1𝑦 + 𝑚̂2𝑦 + 𝑚̂3𝑦
},
where 𝐴 is the area of the element.  Next transverse force equilibrium provides 
1𝑧 = −𝑓 ̂
𝑓 ̂
2𝑧 − 𝑓 ̂
3𝑧.
(10.52)
(10.53)
The corresponding global components of the nodal forces are obtained from the 
following transformation 
⎧𝑓𝑖𝑥
⎫
}
{
𝑓𝑖𝑦
⎬
⎨
}
{
𝑓𝑖𝑧⎭
⎩
=
𝑓𝑖𝑗
𝑙𝑖𝑗
{⎧𝑥𝑖𝑗 + 𝑢𝑖𝑗𝑥
}⎫
𝑦𝑖𝑗 + 𝑢𝑖𝑗𝑦
𝑧𝑖𝑗 + 𝑢𝑖𝑗𝑧 ⎭}⎬
⎩{⎨
+
𝑓𝑖𝑘
𝑙𝑖𝑘
{⎧𝑥𝑖𝑘 + 𝑢𝑖𝑘𝑥
}⎫
𝑦𝑖𝑘 + 𝑢𝑖𝑘𝑦
𝑧𝑖𝑘 + 𝑢𝑖𝑘𝑧 ⎭}⎬
⎩{⎨
+ 𝑓 ̂
𝑖𝑧
{⎧𝑒3𝑥
}⎫
𝑒3𝑦
𝑒3𝑧⎭}⎬
⎩{⎨
. 
(10.54)
Finally, the local moments are transformed to the body coordinates using the relation 
{⎧𝑚̅̅̅̅̅𝑖𝑥
}⎫
𝑚̅̅̅̅̅𝑖𝑦
𝑚̅̅̅̅̅𝑖𝑧⎭}⎬
⎩{⎨
= 𝛌T𝛍
{⎧𝑚̂𝑖𝑥
}⎫
𝑚̂𝑖𝑦
𝑚̂𝑖𝑧⎭}⎬
⎩{⎨
. 
(10.55)
LS-DYNA Theory Manual 
Fully Integrated Shell (Type 16) 
11    
Fully Integrated Shell (Type 16) 
11.1  Introduction 
Shell  type  16  in  LS-DYNA  is  a  fully  integrated  shell  with  assumed  strain 
interpolants  used  to  alleviate  locking  and  enhance  in-plane  bending  behavior,  see 
Engelmann,  Whirley,  and  Goudreau  [1989];  Simo  and  Hughes  [1986];  Pian  and 
Sumihara  [1985].    It  uses  a  local  element  coordinate  system  that  rotates  with  the 
material to account for rigid body motion and automatically satisfies frame invariance 
of the constitutive relations.  The local element coordinate system is similar to the one 
used for the Belytschko-Tsay element, where the the first two basis vectors are tangent 
to the shell midsurface at the center of the element, and the third basis vector is in the 
normal direction of this surface and initially coincident with the fiber vectors.  
11.2  Hu-Washizu Three Field Principle 
The element is derived starting from the Hu-Washizu three-field principle stated 
as 
0 = 𝛿Π(𝐯, 𝐃̅̅̅̅̅ , 𝛔̅̅̅̅̅) = ∫ 𝛿𝐃̅̅̅̅̅ : 𝛔(𝐃̅̅̅̅̅ )𝑑Ω
+ ∫ 𝛿[𝛔̅̅̅̅̅: (𝐃(𝐯) − 𝐃̅̅̅̅̅ )]𝑑Ω
− 𝛿𝑃ext + 𝛿𝑃kin, 
(11.1)
where 𝐯 is the velocity, 𝐃̅̅̅̅̅  is the assumed strain rate, 𝛔̅̅̅̅̅ is the assumed stress, 𝛔 denotes 
the constitutive update as a function of the assumed strain rate, and 𝐃 is the strain rate 
computed  from  the  velocity  field.  𝛿𝑃kin  and  𝛿𝑃ext  are  the  virtual  power  contributions 
from  the  inertial  and  external  forces,  respectively,  and  Ω  denotes  the  domain  of  the 
shell element.  The contribution from the internal forces can be decomposed in the in-
plane and transverse shear parts as 
𝑝 + 𝛿𝑃int
𝑠 + 𝐻𝑝 + 𝐻𝑠 − 𝛿𝑃ext + 𝛿𝑃kin,
0 = 𝛿𝑃int
(11.2)
where
Fully Integrated Shell (Type 16) 
LS-DYNA Theory Manual 
p = ∫ 𝛿𝐃̅̅̅̅̅ p: 𝛔p(𝐃̅̅̅̅̅ )𝑑Ω
𝛿𝑃int
,
𝛿𝑃int
s = 𝜅 ∫ 𝛿𝐃̅̅̅̅̅ s: 𝛔s(𝐃̅̅̅̅̅ )𝑑Ω
,
𝐻p = ∫ 𝛿[𝛔̅̅̅̅̅p: (𝐃p(𝐯) − 𝐃̅̅̅̅̅ p)]𝑑Ω
,
𝐻s = 𝜅 ∫ 𝛿[𝛔̅̅̅̅̅s: (𝐃s(𝐯) − 𝐃̅̅̅̅̅ s)]𝑑Ω
.
(11.3)
(11.4)
(11.5)
(11.6)
Here  κ  is  the  shear  correction  factor  and  the  superscripts  mean  that  only  the  in-plane 
components (p) or transverse shear (s) components are treated. 
11.3  In-plane Assumed Strain Field 
Using  the  standard  isoparametric  interpolation  for  the  four-node  quadrilateral 
element, the in-plane strain rate can be written 
𝐃p = [𝐁m 𝑧𝐁b] [𝐯p
𝛉̇p],
(11.7)
where 𝐁m and 𝐁b are strain-displacement matrices for membrane and bending modes, 
respectively,  𝑧  is  the  through  thickness  coordinate  and  𝐯p  and  𝛉̇p  are  the  nodal  (in-
plane) translational and rotational velocities, respectively. 
To  derive  the  in-plane  assumed  strain  field,  the  interpolants  for  the  assumed 
stress and strain rates are chosen as 
where 
and 
𝛔̅̅̅̅̅p = [𝐒p 𝐒p][
𝐬m
𝐬b
],
𝐃̅̅̅̅̅ p = 𝐂−1[𝐒p 𝐒p][
𝐞m
𝐞b
],
𝐒p =
⎡
⎢⎢
⎣
2𝜂̂
𝑎1
2𝜂̂
𝑎2
𝑎1𝑎2𝜂̂
2𝜉 ̂
𝑏1
⎤
2𝜉 ̂
⎥⎥
, 
𝑏2
𝑏1𝑏2𝜉 ̂⎦
𝜉 ̂ = 𝜉 −
|Ω|
,
∫ 𝜉𝑑Ω
(11.8)
(11.9)
(11.10)
(11.11)
LS-DYNA Theory Manual 
Fully Integrated Shell (Type 16) 
𝜂̂ = 𝜂 −
|Ω|
.
∫ 𝜂𝑑Ω
(11.12)
Furthermore, 𝐂 is the plane stress constitutive matrix and 𝜉  and 𝜂 are the isoparametric 
coordinates.  The coefficients 𝑎𝑖 and 𝑏𝑖 are defined through 
𝐉0 =
[
𝑎1
𝑎2
𝑏1
𝑏2
],
(11.13)
where  𝐉0  is  the  area  jacobian  matrix  from  the  isoparametric  to  physical  domain 
computed at the element center.  
Inserting  the  expressions  for  the  strain  rate  and  assumed  stress  and  strain  rate 
into the expression for 𝐻p and requiring 𝐻p = 0 for arbitrary 𝐬m, 𝐬b, 𝐞m and 𝐞b, yields 
the following expression for the assumed strain rate in terms of the nodal velocities 
𝐃̅̅̅̅̅ p = [𝐁̅̅̅̅̅m 𝑧𝐁̅̅̅̅̅b] [𝐯p
𝛉̇p],
(11.14)
where 
and 
𝐁̅̅̅̅̅m = 𝐂−1𝐒p𝐄̂𝐁̂m,
𝐁̅̅̅̅̅b = 𝐂−1𝐒p𝐄̂𝐁̂b,
𝐄̂ = ∫ 𝐒pT𝐂−1𝐒p𝑑Ω
,
𝐁̂m = ∫ 𝐒pT𝐁m𝑑Ω
,
𝐁̂b = ∫ 𝐒pT𝐁b𝑑Ω
.
(11.15)
(11.16)
(11.17)
(11.18)
(11.19)
11.4  Transverse Shear Assumed Strain Field 
The  transverse  shear  strain  is  the  Bathe-Dvorkin  [1984]  assumed  natural  strain 
field and is derived as follows.  Using the standard isoparametric interpolation for the 
four-node quadrilateral element, the transverse shear strain rate can be written 
𝐯𝑧
𝛉̇𝑝],
where 𝐁𝑡 is the corresponding strain-displacement matrix and 𝐯𝑧 and 𝛉̇𝑝 are the nodal 
out-of-plane translational and in-plane rotational velocities, respectively. 
𝐃s = 𝐁𝑡[
(11.20)
The assumed strain rate is defined as
Fully Integrated Shell (Type 16) 
LS-DYNA Theory Manual 
where 
𝐃̅̅̅̅̅ s = 𝐁̅̅̅̅̅𝑡[
𝐯𝑧
𝛉̇p],
𝐁̅̅̅̅̅𝑡 = 𝐉−T𝐄 ∫ 𝐒𝑠T𝐉T𝐁𝑡𝑑Ω
,
(11.21)
(11.22)
Here  𝐉  is  the  area  jacobian  matrix  from  the  isoparametric  domain  to  the  physical 
domain,  
𝐄 =
[
1 − 𝜉
1 + 𝜉
1 − 𝜂 1 + 𝜂
],
𝐒s = [
δ(η)δ(1 + ξ)
δ(η)δ(1 − ξ)
δ(ξ)δ(1 + η)
δ(ξ)δ(1 − η)
], 
(11.23)
(11.24)
and 𝛿 is the Dirac delta function.  Defining the assumed stress as 
𝛔̅̅̅̅̅p = 𝐉𝐒s𝐬,
(11.25)
yields 𝐻s = 0 regardless of the choice of 𝐬 and thus a B-bar expression for the assumed 
transverse strain rates is obtained as given above.  The result is equivalent to defining 
the isoparametric assumed shear strain rates by interpolating the corresponding strain 
rates from the mid-side points A, B, C and D shown in Figure 11.1. 
Figure 11.1.  Midside locations of isoparametric strain rates
LS-DYNA Theory Manual 
Fully Integrated Shell (Type 16) 
11.5  Rigid Body Motion 
For the in-plane assumed strain field, a rigid body motion may induce a nonzero 
strain rate.  The expression for the in-plane strain rate for a rigid body motion is 
𝐃̅̅̅̅̅ r = 𝐁̅̅̅̅̅r𝛉̇,
where 
𝐁̅̅̅̅̅r = 𝑤𝐁̅̅̅̅̅m𝐑.
(11.26)
(11.27)
11.6  Belytschko-Leviathan Projection 
For warped configurations and since the geometry of the current shell element is 
flat,  extremely  flexible  behavior  can  be  expected  for  some  modes  of  deformation.  
Following [Belytschko and Leviathan 1994], a 7-mode projection matrix 𝐏 (3 rigid body 
rotation modes and 4 nodal drill rotation modes) is constructed used for projecting out 
these zero energy modes.  The explicit formula for the projection matrix is given by  
𝐏 = 𝐈 − 𝐑(𝐑T𝐑)−1𝐑T,
(11.28)
where  𝐑  is  a  matrix  where  each  column  corresponds  to  the  nodal  velocity  of  a  zero 
energy  mode.    This  projection  matrix  operates  on  the  nodal  velocities  prior  to 
computing  the  strain  rates,  and  also  on  the  resulting  internal  force  vector  to  maintain 
invariance of the internal power.
LS-DYNA Theory Manual 
Shells with Thickness Stretch 
12    
Shells with Thickness Stretch 
12.1  Introduction 
Thickness  stretch  is  of  considerable  importance  in  problems  involving  finite  thickness 
strains,  contact  and  surface  loads  in  nonlinear  shell  applications.    As  an  example,  in 
sheet metal forming applications, the presence of normal stresses in thickness direction 
improves the accuracy of the solution and also its response on the double sided contact 
zone between dies and sheet. It has also been shown that a kinematical representation 
of a continuous thickness field improves the instability characteristics when  compared 
to experimental results, see Figure Figure 1212-1 and Björklund [2014]. 
There  have  been  several  attempts  to  account  for  the  through-thickness  deformation  in 
the  literature,  this  implementation  is  inspired  by  the  7P-CYSE  shell  introduced  in 
Cardoso and Yoon [2005]. However, the formulation in this paper is rather complicated 
and  involves  for  instance  assumed  shear  strains  (ANS)  to  alleviate  shear  locking  and 
complicated setup of internal forces and stiffness matrices by combined analytical and 
numerical integration to restore rank deficiencies. A direct implementation of this shell 
following  the  theory  was  ruled  out  for  efficiency  reasons,  and  another  approach  was 
taken in order to presumably get a useful shell. 
The  Belytschko-Tsay  shell  element  is  one  of  the  fastest  elements  for  thin  shell 
simulations.  This, together with its robustness, is the reason why it is popular in finite 
element codes.  The implementation of shell type 25, the reduced integrated shell with 
thickness  stretch,  is  based  on  the  formulation  of  the  Belytschko-Tsay  shell  with  a 
relaxation of the thickness variable.  This ensures that it will be efficient and hopefully 
also possess properties useful for applications where through thickness deformation is 
important.    As  a  fully  integrated  alternative,  shell  type  26  is  available  as  an  analogue 
extension of shell type 16 (fully integrated Belytschko-Tsay), and a triangular shell with 
thickness  stretch  is  available  as  type  27  mainly  to  allow  for  hybrid  meshes  (quadrilat-
erals combined with triangles) in this context. 
The  theory  that  follows  is  very  similar  to  that  of  the  Belytschko-Tsay  (type  2),  Fully 
Integrated  Shell  (type  16)  and  C0-shell  (type  4),  and  here  we  emphasize  on  the  parts 
involving the amendments to those shell formulations.
Shells with Thickness Stretch 
LS-DYNA Theory Manual 
Shell  16,  no  transverse  shear 
discontinuous 
and 
stress 
thickness field
Shell 26, transverse shear stress 
and continuous thickness field 
25
20
15
10
]
[
,
0.5
Experiment
Plane Stress
With Normal Stress
2.5
1.5
Displacement, δ [mm]
Figure 1212-1 Example of premature localization with shell type 16 
while  shell  type  26  matches  experimental  result  (from  Björklund 
12.2  Shell Type 25 
12.2.1  Formulation 
The  kinematics,  i.e.,  position  𝒙  and  velocity  𝒗,  of  a  material  point  in  the  shell  with 
through thickness stretch can be written in the shell element local coordinate system as 
(sum over nodal indices 𝐼) 
where we have set 
𝒙 = (𝒙𝐼 + 𝑠𝐼𝒏)𝑁𝐼(𝜉 , 𝜂)
𝒗 = (𝒗𝐼 + 𝑠𝐼𝝎𝐼 × 𝒏 + 𝑠 ̇𝐼𝒏)𝑁𝐼(𝜉 , 𝜂)
𝑠𝐼 =
𝑡𝐼 + (1 − 𝜍2)𝑞𝐼.
(12.1)
(12.2)
The  kinematics  is  based  on  the  Belytschko-Tsay  shell  with  the  additional  feature  that 
the  thickness  is  variable,  whence  the  last  term  in  the  second  of  (12.1).  The  thickness 
variable  is  represented  by  𝑡𝐼  and  an  additional  strain  variable  𝑞𝐼  to  allow  for  a  linear 
strain through the thickness.  The latter represents the location of the mid-surface and is 
important to avoid “Poisson locking” in bending modes of deformation, so the shell has 
two  additional  degrees  of  freedom  compared  to  the  Belytschko-Tsay  shell.  The  other 
variables  and  parameters  are  the  nodal  coordinates  𝒙𝐼,  nodal  velocities  𝒗𝐼,  nodal 
1)𝑇  and  bilinear  isoparametric  shape 
rotational  velocities  𝝎𝐼,  shell  normal  𝒏 = (0
functions 𝑁𝐼. From this we can determine the local velocity gradient as  
𝜕𝒗
𝜕𝒙
= (𝒗𝐼 + 𝑠𝐼𝝎𝐼 × 𝒏 + 𝑠 ̇𝐼𝒏)
𝜕𝑁𝐼
𝜕𝒙
+ (𝝎𝐼 × 𝒏
𝜕𝑠𝐼
𝜕𝒙
+ 𝒏
𝜕𝑠 ̇𝐼
𝜕𝒙
) 𝑁𝐼. 
(12.3)
LS-DYNA Theory Manual 
Shells with Thickness Stretch 
In the local system one can assume a vanishing third component of both 𝝎𝐼 × 𝒏 and 
and the thickness strain rate is given by 
𝜕𝑁𝐼
𝜕𝒙 , 
𝜀̇𝑡 =
𝜕𝑠 ̇
𝜕𝑥3
=
𝑡 ̇− 4𝜍𝑞 ̇
𝑡 − 4𝜍𝑞
(12.4)
where  we  used  the  notation  𝑠 = 𝑠𝐼𝑁𝐼,  𝑡 = 𝑡𝐼𝑁𝐼  and  𝑞 = 𝑞𝐼𝑁𝐼,  sum  over  𝐼.  For  small 
strains 𝑞 = 0, and this shows that the thickness strain rate is at most linear. 
For  evaluating  internal  forces  we  define  the  strain-displacement  tensor  through 
(assuming Voigt notation and sum over 𝐼) 
𝜕𝒗
𝜕𝒙
= 𝑩𝐼𝒖𝐼 ,
(12.5)
and the nodal vector 𝒖𝐼 is given by 
𝑡 ̇𝐼
indicating the 8 degrees of freedom per node in these elements.  The principle of virtual 
work results in an internal force vector 
𝒖𝐼 = (𝒗𝐼
𝑇 𝝎𝐼
𝑞 ̇𝐼)𝑇 ,
(12.6)
𝒇𝐼 = ∫ 𝑩𝐼
𝑇𝝈 ,
(12.7)
where 𝝈 is the Cauchy stress and the integral is over the current element configuration. 
12.2.2  Hourglass modes 
Shell  type  25  is  a  reduced  integration  element  and  in  addition  to  the  six  hourglass 
modes  present  in  the  original  Belytschko-Tsay  shell,  two  more  are  added  by  the 
introduction  of  the  thickness  variables.    Fortunately  these  are  orthogonal  to  any  rigid 
body motion and/or any other hourglass mode, and are given by 
where 
𝑡𝐼 = ℎ𝐼
𝑞𝐼 = ℎ𝐼
ℎ𝐼 = (−1)𝐼/4
(12.8)
(12.9)
and  all  other  displacement  components  are  zero.    To  restrain  these  modes  we  have 
included generalized strains and stresses according to the following (sum over 𝐼) 
ℎ =
𝜀̇𝑡
ℎ = −
𝜀̇𝑞
ℎ𝐼𝑡 ̇𝐼
4ℎ𝐼𝑞 ̇𝐼
The corresponding generalized stresses are obtained through 
𝜎̇𝑡 = 𝐸𝐻𝜀̇𝑡
(12.10)
(12.11)
Shells with Thickness Stretch 
LS-DYNA Theory Manual 
and the forces are then given by 
𝜎̇𝑞 =
𝐸𝐻
𝜀̇𝑞
𝑡 = 𝐴ℎ𝐼𝜎𝑡
𝑓𝐼
𝑞 = −4𝐴ℎ𝐼𝜎𝑞
𝑓𝐼
(12.12)
where 𝐴 is the area of the element and the value of 𝐸𝐻 is taken as 𝐸𝐻 = 0.05𝐸, i.e., 5% of 
the Young’s modulus. 
12.3  Shell Type 26 
12.3.1  Modifying shell type 16 
When using full integration, care must be taken in order to avoid the well-known shear 
locking phenomenon.  Common techniques developed for this are the ANS (Assumed 
Natural  Strain)  and  various  types  of  EAS  (Enhanced  Assumed  Strain)  techniques.    In 
Cardoso  and  Yoon  [2004]  the  ANS  technique  is  used  in  which  the  transverse  shear 
strains  are  interpolated  from  the  mid  points  of  the  shell  element  edges.    It  is  reported 
that this is a successful technique, but when consulting Bischoff and Ramm [1997] it is 
reported  that  it  is  not  well  suited  to  avoid  membrane  locking  and  reduce  mesh 
distortion  sensitivity.    They  are  proposing  a  combination  of  ANS  and  EAS  to  get  a 
decent  shell  element  formulation.    However,  elements  that  use  an  EAS  in  general 
require  a  nonlinear  solution  for  the  assumed  strain  variables  which  can  be  computa-
tionally rather expensive. The approach taken here is to suitably modifying an existing 
LS-DYNA  standard  assumed  strain  element,  i.e.,  element  type  16,  which  is  a  fully 
integrated extension of the Belytschko-Tsay element.  Due to the rather complex setup 
of assumed strain components, we use the following in order to extend the element to 
variable  thickness  stretch  without  having  to  bother  about  all  the  details  of  the 
kinematics. 
In the beginning of a time step, the thickness components are reset to the corresponding 
value in the center of the shell element.  That is 
𝑠 ̃ =
𝑠1 + 𝑠2 + 𝑠3 + 𝑠4
(12.13)
is  used  for  evaluating  the  strain  increments.    However,  the  rates  of  the  thickness 
variables  are  unchanged,  so  this  can  be  seen  as  an  assumed  strain  approach  in  the 
thickness  direction.  Using  this,  the  velocity gradient  expression  is  an  augmentation  of 
that of element 16 
𝜕𝒗
𝜕𝒙
=
𝜕𝒗
𝜕𝒙
∣
16
+ 𝑠 ̇𝐼𝒏
𝜕𝑁𝐼
𝜕𝒙
+ 𝒏
𝜕𝑠 ̇𝐼
𝜕𝒙
𝑁𝐼.
(12.14)
This should be interpreted that the velocity gradient used in shell element type 16 as a 
function  of  the  current  thickness  coordinate  𝑠 ̃  (and  its  isoparametric  derivative)  is
LS-DYNA Theory Manual 
Shells with Thickness Stretch 
augmented  by  thickness  component  rates.  Furthermore,  to  avoid  locking  phenomena 
and  still  maintaining  a  non-singular  element  we  use  single  point  integration  of  the 
thickness  strain  component  and  an  ANS  approach  for  the  transverse  shear  strain 
components  emanating  from  the  rates  of  thickness  components.  This  approach  is 
inspired by the methodology used for the Belytschko-Tsay shell in which the nodal fiber 
vectors are reset in the beginning of each time step, and in an analogous way we reset 
the  thickness  components  in  the  beginning  of  each  time  step  in  this  shell  element 
formulation.  
12.4  Shell Type 27 
12.4.1  Modifying shell type 4 
A  triangular  element  with  thickness  stretch  was  added  to  allow  consistent  sorting  of 
triangular  shell  elements,  and  not  necessarily  intended  to  be  used  for  other  purposes. 
The  approach  taken  is  very  similar  to  that  of  shell  type  26,  the  existing  LS-DYNA 
standard  C0  triangular  element  was  modified  according  to  the  same  principles  as 
described  in  the  previous  section.    In  this  case  the  velocity  gradient  expression  is 
modified according to 
𝜕𝒗
𝜕𝒙
=
𝜕𝒗
𝜕𝒙
∣
+ 𝒏
𝜕𝑠 ̃
𝜕𝒙
(12.15)
where  again  the  subindex  4  indicates  that  it’s  the  velocity  gradient  of  element  type  4 
evaluated with respect to the average thickness value 𝑠 ̃ and its isoparametric derivative. 
For  the  triangular  element  type  27  the  thickness  is  always  constant  in  the  element,  a 
decision that was taken for the sake of simplicity. More on thickness distribution in the 
next section. 
12.5  Related Features 
12.5.1  Continuous vs decoupled thickness field 
A  drawback  with  having  a  continuous  thickness  field  is  that  complicated  geometries 
tend  to  lock  the  structure.    This  approach  assumes  that  the  geometry  is  relatively  flat 
and  may  be  suitable  in  metal  forming  but  not  in  other  situations.  To  remedy  this  we 
added the option to decouple the thickness field so that the thickness is discontinuous 
between elements, which makes the element suitable for crash analysis.  To activate this 
option the user should put the variable IDOF on *SECTION_SHELL equal to 2, which 
actually  is  the  default.  For  shell  element  type  25,  this  option  will  make  the  thickness 
variable  constant  in  the  element,  and  the  implementation  follows  the  one  described 
above with the restriction  𝑡𝐼 = 𝑡  (constant)  and  𝑞𝐼 = 𝑞  (constant).  No  additional  zero 
energy modes are present with this approach. 
LS-DYNA Draft
Shells with Thickness Stretch 
LS-DYNA Theory Manual 
Using the same approach for element type 26 turns out to be a poor choice since it leads 
to locking phenomenon due to full integration.  Instead we use the approach where the 
thickness is bilinear within but discontinuous between elements, which turns out to be 
successful.  That means that the same code can be executed regardless of the choice of 
IDOF for this element. 
12.5.2  Nodal masses 
For dynamic analysis some mass quantity must be associated with the extra degrees of 
freedom,  and  although  a  consistent  finite  element  approach  is  applicable  the  mass  is 
here empirically estimated from elaborating with the kinetic energy for compressive in-
plane and out-of-plane modes.  That is, the kinetic energy of an in-plane uniaxial strain 
mode  should  have  the  same  kinetic  energy  as  the  equivalent  out-of-plane  ditto.  This 
assumption  leads  to  a  mass  of  the  scalar  nodes  given  by  𝑚 = 𝑚𝑇/4  where  𝑚𝑇  is  the 
translational mass. A problem with this approach is that it leads to instabilities due to 
high eigenfrequencies of the shell.  For this reason we have set  
3𝐴
2𝑡2)𝑚𝑇
where 𝐴 is the element area and 𝑡 is the thickness. 
𝑚 = max(1,
𝒇  
(12.16)
𝑡 
Figure 1212-2 Contact influence on thickness stretch shells. 
−𝒇
12.5.3  Transfer of contact forces 
The new degrees of freedom allows for a different treatment of how contact forces are 
transferred  from  master  to  slave,  for  this  discussion  we  refer  to  Figure  Figure  1212-2. 
The  nodal  forces  in  local  system  acting  on  the  slave  from  contact  on  the  upper  and 
lower surface can roughly be written
LS-DYNA Theory Manual 
Shells with Thickness Stretch 
𝑢/𝑙 = (±
𝒇𝐼
𝒇 𝑇
(𝒏 ×
)
𝑇 𝒏 ∙ 𝒇
0)
(12.17)
where  we  used  the  same  order  of  the  degrees  of  freedom  as  in  (12.6).  Summing  these 
two force contributions give nodal contact forces acting on the slave given by 
𝑐 = (𝟎𝑇
𝒇𝐼
𝑡 (𝒏 ×
)
𝑇 𝒏 ∙ 𝒇
0)
(12.18)
We  can  see  that  the  total  force  include  nodal  moments  caused  by  the  frictional  forces 
acting  at  an  offset  from  the  midsurface  of  the  shell,  but  also  a  pressure  acting  on  the 
thickness  degree  of  freedom.    In  conclusion,  the  relaxation  of  the  thickness  in  the 
Belytschko-Tsay shell allows for double sided contact zones, i.e., the shell is affected by 
contact pressure from both sides even though they are of equal magnitude.  This is not 
possible in traditional shell with zero normal stress, unless a modified option is used. 
12.6  Contact Pressure Treatment in Shells 2, 4 and 16 
By  specifying  IDOF = 3  on  *SECTION_SHELL  for  the  Belytschko-Tsay  (type  2),  C0-
element (type 4) and Fully Integrated (type 16) shell, the contact pressure influences the 
stress  and  can  induce  thickness  changes.  This  is  a  short  explanation  of  the  theory 
behind. 
The z-stress in a shell element is usually restricted to be zero, but in this case we intend 
to solve the constitutive update using the constraint 
where  
and 
𝜎𝑧𝑧 = 𝛼𝜎𝑐(𝑧)
𝜎𝑐(𝑧) = −
𝑏 − 𝜎𝑐
𝜎𝑐
(𝑧3 − 3𝑧) −
𝑏 + 𝜎𝑐
𝜎𝑐
(12.19)
(12.20)
𝑏= contact pressure at bottom surface of shell 
𝑡= contact pressure at top surface of shell 
𝜎𝑐
𝜎𝑐
𝑧= isoparametric coordinate through the thickness between -1 and 1 
𝛼= scaling parameter 
The  scaling  parameter  can  be  set  as 
*CONTROL_CONTACT. 
The constitutive update for en elastic-plastic material can be written 
the  8th  parameter  on  card  3  on 
𝛔𝑛+1 = 𝛔𝑛 + 𝐾∆𝜀𝑣𝑜𝑙𝐈 + ∆𝐬(𝐬𝑛, ∆𝛆𝑑𝑒𝑣) 
𝑛+1 = 𝜎𝑐
𝜎𝑧𝑧
𝑛+1 
(12.21)
(12.22)
where
Shells with Thickness Stretch 
LS-DYNA Theory Manual 
𝛔𝑛+1 = stress in step n+1 
𝛔𝑛 = stress in step n 
𝐾= bulk modulus 
∆𝛆 = strain increment 
∆𝜀𝑣𝑜𝑙 = ∆𝛆: 𝐈 = volumetric strain increment 
𝐈 = unit tensor 
∆𝐬= deviatoric stress increment 
𝐬𝑛 = 𝛔𝑛 − 𝛔𝑛:𝐈 
∆𝛆𝑑𝑒𝑣 = ∆𝛆 − ∆𝛆: 𝐈
3 𝐈 = deviatoric stress in step n 
3  𝐈 = deviatoric strain increment 
The  independent  variables  in  (12.21)  and  (12.22)  are  𝜎𝑥𝑥
∆𝜀𝑧𝑧. 
Here  we  assume  that  the  stress  response  can  be  decoupled  into  a  volumetric  and 
deviatoric part and the deviatoric stress increment depends only on the deviatoric part 
of  the  stress  and  strain  increment  as  indicated  in  the  formula.    We  can  rewrite  (12.21) 
and (12.22) as 
𝑛+1, 𝜎𝑦𝑦
𝑛+1, 𝜎𝑥𝑦
𝑛+1, 𝜎𝑦𝑧
𝑛+1  and 
𝑛+1, 𝜎𝑥𝑧
by substituting 
and 
𝛔̃𝑛+1 = 𝛔̃𝑛 + 𝐾∆𝜀̃𝑣𝑜𝑙𝐈 + ∆𝐬(𝐬̃𝑛, ∆𝛆̃𝑑𝑒𝑣)
𝑛+1 = 0 
𝜎̃𝑧𝑧
𝑛𝐈
𝛔̃𝑛 = 𝛔𝑛 − 𝜎𝑐
𝛔̃𝑛+1 = 𝛔𝑛+1 − 𝜎𝑐
𝑛+1𝐈 
∆𝛆̃ = ∆𝛆 −
𝑛+1 − 𝜎𝑐
𝜎𝑐
3𝐾
𝐈.
Since the deviatoric stress and strain increment is not changed, i.e., 
𝐬𝑛 = 𝐬̃𝑛
∆𝛆𝑑𝑒𝑣 = ∆𝛆̃𝑑𝑒𝑣 
(12.23)
(12.24)
(12.25)
(12.26)
(12.27)
(12.28)
(12.29)
with  this  substitution  it  follows  that  the  existing  material  routines  can  be  used  for 
𝑛+1 and ∆𝜀̃𝑧𝑧 and then use 
𝑛+1, 𝜎̃𝑦𝑦
solving (12.23) and (12.24) in terms of 𝜎̃𝑥𝑥
the  inverse  of  (12.26)  and  (12.27)  to  establish  the  stress  and  through  thickness  strain 
increment.  Thus, the algorithm is as follows 
𝑛+1, 𝜎̃𝑥𝑦
𝑛+1, 𝜎̃𝑦𝑧
𝑛+1, 𝜎̃𝑥𝑧
𝑛+1  
𝑛 and 𝜎𝑐
1.Given 𝛔𝑛, ∆𝛆, 𝜎𝑐
2.Use (12.25) and (12.27) to compute  𝛔̃𝑛 and ∆𝛆̃. 
3.Do a constitutive update, (12.23) and (12.24), to get  𝛔̃𝑛+1 and ∆𝜀̃𝑧𝑧. 
4.Use (12.26) and (12.27) to compute 𝛔𝑛+1  and ∆𝜀𝑧𝑧.
LS-DYNA Theory Manual 
Shells with Thickness Stretch 
Figure  1212-3  Compression  of  a  shell  sheet  between  two  rigid 
plates using IDOF = 3 on shell 16.
LS-DYNA Theory Manual 
Hughes-Liu Shell 
13    
Hughes-Liu Shell 
The Hughes-Liu shell element formulation ([Hughes and Liu 1981a, b], [Hughes 
et  al.,  1981],  [Hallquist  et  al.,  1985])  was  the  first  shell  element  implemented  in  LS-
DYNA.    It  was  selected  from  among  a  substantial  body  of  shell  element  literature 
because the element formulation has several desirable qualities: 
•  it  is  incrementally  objective  (rigid  body  rotations  do  not  generate  strains), 
allowing for the treatment of finite strains that occur in many practical applica-
tions; 
•  it  is  simple,  which  usually  translates  into  computational  efficiency  and  robust-
ness; 
•  it is compatible with brick elements, because the element is based on a degener-
ated brick element formulation.  This  compatibility allows many of the efficient 
and  effective  techniques  developed  for  the  DYNA3D  brick  elements  to  be  used 
with this shell element; 
•  it includes finite transverse shear strains; 
•  a through-the-thickness thinning option  is also 
available when needed in some shell element applications. 
The remainder of this section reviews the Hughes-Liu shell element (referred to 
by  Hughes  and  Liu  as  the  U1  element)  which  is  a  four-node  shell  with  uniformly 
reduced  integration,  and  summarizes  the  modifications  to  their  theory  as  it  is 
implemented  in  LS-DYNA.    A  detailed  discussion  of  these  modifications,  as  well  as 
those associated with the implementation of the Hughes-Liu shell element in NIKE3D, 
are presented in an article by Hallquist and Benson [1986].
Hughes-Liu Shell 
LS-DYNA Theory Manual 
13.1  Geometry 
The Hughes-Liu shell element is based on a degeneration of the standard 8-node 
brick element formulation, an approach originated by Ahmad et al. [1970].  Recall from 
the discussion of the solid elements the isoparametric mapping of the biunit cube: 
𝐱(𝜉 , 𝜂, 𝜁 ) = 𝑁𝑎(𝜉 , 𝜂, 𝜁 )𝐱𝑎,
𝑁𝑎 (𝜉 , 𝜂, 𝜁 ) =
(1 + 𝜉𝑎𝜉 )(1 + 𝜂𝑎𝜂)(1 + 𝜁𝑎𝜁 )
,
(13.1)
(13.2)
where 𝐱 is an arbitrary point in the element, (𝜉 , 𝜂, 𝜁 ) are the parametric coordinates, 𝐱𝑎 
are  the  global  nodal  coordinates  of  node  𝑎,  and  𝑁𝑎  are  the  element  shape  functions 
evaluated at node 𝑎, i.e., (𝜉𝑎, 𝜂𝑎, 𝜁𝑎) are (𝜉 , 𝜂, 𝜁 ) evaluated at node 𝑎. 
In the shell geometry, planes of constant 𝜁  will define the lamina or layers of the 
shell  and  fibers  are  defined  by  through-the-thickness  lines  when  both  𝜉   and  𝜂  are 
constant  (usually  only  defined  at  the  nodes  and  thus  referred  to  as  ‘nodal  fibers’).    To 
degenerate the 8-node brick geometry into the 4-node shell geometry, the nodal pairs in 
the  𝜁   direction  (through  the  shell  thickness)  are  combined  into  a  single  node,  for  the 
translation  degrees  of  freedom,  and  an  inextensible  nodal  fiber  for  the  rotational 
degrees  of  freedom.    Figure  13.1  shows  a  schematic  of  the  bi-unit  cube  and  the  shell 
element. 
The mapping of the bi-unit cube into the shell element is separated into two parts 
𝐱(𝜉 , 𝜂, 𝜁 ) = 𝐱̅(𝜉 , 𝜂) + 𝐗(𝜉 , 𝜂, 𝜁 ),
(13.3)
where 𝐱̅ denotes a position vector to a point on the reference surface of the shell and X is 
a  position  vector,  based  at  point  𝐱̅  on  the  reference,  that  defines  the  fiber  direction 
through that point.  In particular, if we consider one of the four nodes which define the 
reference surface, then 
𝐱̅ (𝜉 , 𝜂) = 𝑁𝑎 (𝜉 , 𝜂) 𝐱̅𝑎,
𝐗(𝜉 , 𝜂, 𝜁 ) = 𝑁𝑎 (𝜉 , 𝜂)𝐗𝑎(𝜁 ).
(13.4)
(13.5)
With this description, arbitrary points on the reference surface 𝐱̅ are interpolated 
by the two-dimensional shape function 𝑁(𝜉 , 𝜂) operating on the global position of the 
four  shell  nodes  that  define  the  reference  surfaces,  i.e.,  𝐱̅𝑎.    Points  off  the  reference 
surface  are  further  interpolated  by  using  a  one-dimensional  shape  function  along  the 
fiber direction, i.e., 𝐗𝑎(𝜁 ), where 
𝐗𝑎(𝜁 ) = 𝑧𝑎(𝜁 ) 𝐗̂𝑎,
𝑧𝑎(𝜁 ) = 𝑁+(𝜁 )𝑧𝑎
−,
+ + 𝑁−(𝜁 )𝑧𝑎
(13.6)
(13.7)
LS-DYNA Theory Manual 
Hughes-Liu Shell 
Biunit Cube
Beam Element
Nodal fibers
Top Surface
z+
x+
x^
x¯
x^
x-
Bottom Surface
z-
+1
ζ¯
-1
Figure  13.1.    Mapping  of  the  biunit  cube  into  the  Hughes-Liu  shell  element 
and nodal fiber nomenclature. 
𝑁+(𝜁 ) =
𝑁−(𝜁 ) =
(1 + 𝜁 )
,
(1 − 𝜁 )
(13.8)
(13.9)
As  shown  in  the  lower  portion  of Figure  13.1,  𝐗̂𝑎  is  a  unit vector  in  the  fiber  direction 
and  𝑧(𝜁 )  is  a  thickness  function.    (Thickness  changes   
are  accounted  for  by  explicitly  adjusting  the  fiber  lengths  at  the  completion  of  a  time 
step based on the amount of straining in the fiber direction.  Updates of the fiber lengths 
always lag one time step behind other kinematical quantities.) 
The reference surface may be located at the mid-surface of the shell or at either of 
the  shell’s  outer  surfaces.    This  capability  is  useful  in  several  practical  situations 
involving contact surfaces, connection of shell elements to solid elements, and offsetting 
elements such as stiffeners in stiffened shells.  The reference surface is located within the 
shell  element  by  specifying  the  value  of  the  parameter  𝜁 ̅  (see  lower  portion  of  Figure
Hughes-Liu Shell 
LS-DYNA Theory Manual 
13.1).  When  𝜁 ̅ = – 1, 0, +1,  the  reference  surface  is  located  at  the  bottom,  middle,  and 
top surface of the shell, respectively. 
The Hughes-Liu formulation uses two position vectors, in addition to 𝜁 ̅, to locate 
+ 
the reference surface and define the initial fiber direction.  The two position vectors 𝑥𝑎
− are located on the top and bottom surfaces, respectively, at node 𝑎.  From these 
and 𝑥𝑎
data the following are obtained: 
𝑥̅𝑎   =
(1 − 𝜁 ̅)𝑥𝑎
+,
− + (1 + 𝜁 ̅)𝑥𝑎
𝑋̂𝑎 =
(𝑥𝑎
−)
+ − 𝑥𝑎
ℎ𝑎
,
+ =
𝑧𝑎
(1 − 𝜁 ̅)ℎ𝑎,
− = −
𝑧𝑎
(1 + 𝜁 ̅)ℎ𝑎,
ℎ𝑎 = ∥𝑥𝑎
+ − 𝑥𝑎
−∥,
(13.10)
(13.11)
(13.12)
(13.13)
(13.14)
where ‖ ⋅ ‖ is the Euclidean norm. 
13.2  Kinematics 
The  same  parametric  representation  used  to  describe  the  geometry  of  the  shell 
element, i.e., reference surface and fiber vector interpolation, are used to interpolate the 
shell  element  displacement, 
  Again,  the 
displacements  are  separated  into  the  reference  surface  displacements  and  rotations 
associated with the fiber direction: 
isoparametric  representation. 
i.e.,  an 
𝐮(𝜉 , 𝜂, 𝜁 ) = 𝐮̅̅̅̅(𝜉 , 𝜂) + 𝐔(𝜉 , 𝜂, 𝜁 ),
𝐮̅̅̅̅(𝜉 , 𝜂) = 𝑁𝑎(𝜉 , 𝜂)𝐮̅̅̅̅𝑎,
𝐔(𝜉 , 𝜂, 𝜁 ) = 𝑁𝑎(𝜉, 𝜂)𝐔𝑎(𝜁 ),
𝐔𝑎(𝜁 ) = 𝑧𝑎(𝜁 )𝐔̂𝑎,
(13.15)
(13.16)
(13.17)
(13.18)
where 𝐮 is the displacement of a generic point; 𝐮̅̅̅̅ is the displacement of a point on the 
reference  surface,  and  𝐔  is  the  ‘fiber  displacement’  rotations;  the  motion  of  the  fibers 
can be interpreted as either displacements or rotations as will be discussed.
LS-DYNA Theory Manual 
Hughes-Liu Shell 
Hughes  and  Liu  introduce  the  notation  that  follows,  and  the  associated 
schematic  shown  in  Figure  13.2,  to  describe  the  current  deformed  configuration  with 
respect to the reference configuration: 
𝐲 = 𝐲̅̅̅̅ + 𝐘,
𝐲̅̅̅̅ = 𝐱̅ + 𝐮̅̅̅̅,
𝐲̅̅̅̅𝑎 = 𝐱̅𝑎 + 𝐮̅̅̅̅𝑎,
𝐘 = 𝐗 + 𝐔,
𝐘𝑎 = 𝐗𝑎 + 𝐔𝑎,
𝐘̂𝑎 = 𝐗̂𝑎 + 𝐔̂𝑎.
(13.19)
(13.20)
(13.21)
(13.22)
(13.23)
(13.24)
In  the  above  relations,  and  in  Figure  13.2,  the  𝐱  quantities  refer  to  the  reference 
configuration, the 𝐲 quantities refer to the updated (deformed) configuration and the 𝐮 
quantities are the displacements.  The notation consistently uses a superscript bar (⋅ ̅) to 
indicate  reference  surface  quantities,  a  superscript  caret  (⋅ ̂)  to  indicate  unit  vector 
quantities,  lower  case  letters  for  translational  displacements,  and  upper  case  letters 
indicating  fiber  displacements.    To  update  to  the  deformed  configuration,  two  vector 
quantities  are  needed:    the  reference  surface  displacement  𝐮̅̅̅̅  and  the  associated  nodal 
fiber displacement 𝐔.  The nodal fiber displacements are defined in the fiber coordinate 
system, described in the next subsection. 
13.2.1  Fiber Coordinate System 
For  a  shell  element  with  four  nodes,  the  known  quantities  will  be  the 
displacements  of  the  reference  surface  𝐮̅̅̅̅  obtained  from  the  translational  equations  of 
motion  and  some  rotational  quantities  at  each  node  obtained  from  the  rotational 
equations  of  motion.    To  complete  the  kinematics,  we  now  need  a  relation  between 
nodal rotations and fiber displacements 𝐔.
Hughes-Liu Shell 
LS-DYNA Theory Manual 
(parallel construction)
u¯
reference axis in
undeformed 
geometry
Deformed Configuration
Reference Surface
x¯
Figure 13.2.  Schematic of deformed configuration displacements and position
vectors. 
At  each  node  a  unique  local  Cartesian  coordinate  system  is  constructed  that  is 
used  as  the  reference  frame  for  the  rotation  increments.    The  relation  presented  by 
Hughes and Liu for the nodal fiber displacements (rotations) is an incremental relation, 
i.e., it relates the current configuration to the last state, not to the initial configuration.  
𝑓 )  comprising  the  orthonormal 
Figure  13.3  shows  two  triads  of  unit  vectors:  (𝐛1
𝑓 ) and 
fiber basis in the reference configuration (where the fiber unit vector is now 𝐘̂ = 𝐛3
(𝐛1, 𝐛2, 𝐛3)  indicating  the  incrementally  updated  current  configuration  of  the  fiber 
 and 
vectors.  The reference triad is updated by applying the incremental rotations, Δ𝜃1
 𝑓 ) 
Δ𝜃2, obtained from the rotational equations of motion, to the fiber vectors (𝐛 1
as shown in Figure 13.3.  The linearized relationship between the components of Δ𝑈̂ in 
the fiber system viz, Δ𝑈̂
𝑓 , and the incremental rotations is given by 
 𝑓 and  𝐛 2
𝑓 , Δ𝑈̂
𝑓 , 𝐛2
𝑓 , 𝐛3
𝑓 ,  Δ𝑈̂
⎧Δ𝑈̂
{{
Δ𝑈̂
⎨
{{
Δ𝑈̂
⎩
⎫
}}
⎬
}}
⎭
   =
−1
⎢⎡
⎣
0 −1
0 ⎦
⎥⎤  {
Δ𝜃1
Δ𝜃2
}. 
(13.25)
Although the above Hughes-Liu relation for updating the fiber vector enables a 
reduction  in  the  number  of  nodal  degrees  of  freedom  from  six  to  five,  it  is  not 
implemented in LS-DYNA because it is not applicable to beam elements.
LS-DYNA Theory Manual 
Hughes-Liu Shell 
fiber
^
f =Y
b3
b3
Δθ
b1
b1
b2
b2
Δθ
Figure  13.3. 
incremental rotations. 
  Incremental  update  of  fiber  vectors  using  Hughes-Liu 
In LS-DYNA, three rotational increments are used, defined with reference to the 
global coordinate axes: 
{{⎧Δ𝑈̂1
}}⎫
Δ𝑈̂2
}}⎬
⎩{{⎨
Δ𝑈̂3⎭
  =
𝑌̂3 −𝑌̂2
⎤
⎡
−𝑌̂3
𝑌̂1
⎥⎥
⎢⎢
𝑌̂2 −𝑌̂1
0 ⎦
⎣
{⎧Δ𝜃1
}⎫
Δ𝜃2
Δ𝜃3⎭}⎬
⎩{⎨
. 
(13.26)
Equation  (13.26)  is  adequate  for  updating  the  stiffness  matrix,  but  for  finite 
rotations the error is significant.  A more accurate second-order technique is used in LS-
DYNA for updating the unit fiber vectors: 
𝑌̂
𝑛+1 = 𝑅𝑖𝑗(Δ𝜃)𝑌̂𝑖
𝑛,
𝑅𝑖𝑗(Δ𝜃) = 𝛿𝑖𝑗 +
(2𝛿𝑖𝑗 + Δ𝑆𝑖𝑘)Δ𝑆𝑖𝑘
,
ΔS𝑖𝑗 = e𝑖𝑘𝑗Δ𝜃𝑘,
2𝐷 = 2 +
(Δ𝜃1
2 + Δ𝜃2
2 + Δ𝜃3
2).
(13.27)
(13.28)
(13.29)
(13.30)
Here, 𝛿𝑖𝑗 is the Kronecker delta and 𝑒𝑖𝑗𝑘 is the permutation tensor.  This rotational update 
is often referred to as the Hughes-Winget formula [Hughes and Winget 1980].  An exact 
rotational update using Euler angles or Euler parameters could easily be substituted in 
Equation (13.27), but it is doubtful that the extra effort would be justified. 
13.2.2  Lamina Coordinate System 
In  addition  to  the  above  described  fiber  coordinate  system,  a  local  lamina 
coordinate  system  is  needed  to  enforce  the  zero  normal  stress  condition,  i.e.,  plane
Hughes-Liu Shell 
LS-DYNA Theory Manual 
nt
nsta
ξ = co
e^
η = constant
e^
e^
Figure 13.4.  Schematic of lamina coordinate unit vectors. 
stress.    Lamina  are  layers  through  the  thickness  of  the  shell  that  correspond  to  the 
locations  and  associated  thicknesses  of  the  through-the-thickness  shell  integration 
points; the analogy is that of lamina in a fibrous composite material.  The orthonormal 
lamina  basis  (Figure  13.4),  with  one  direction  𝑒 ̂3  normal  to  the  lamina  of  the  shell,  is 
constructed at every integration point in the shell. 
The lamina basis is constructed by forming two unit vectors locally tangent to the 
lamina: 
𝐞̂1 =
𝐞′2 =
𝐲,𝜉
∥𝐲,𝜉 ∥
,
𝐲,𝜂
∥𝐲,𝜂 ∥
,
(13.31)
(13.32)
where, as before, 𝐲 is the position vector in the current configuration.  The normal to the 
lamina  at  the  integration  point  is  constructed  from  the  vector  cross  product  of  these 
local tangents: 
𝐞̂3 = 𝐞̂1 × 𝐞′2,
𝐞̂2 = 𝐞̂3 × 𝐞̂1,
(13.33)
(13.34)
is defined, because 𝐞̂2, although tangent to both the lamina and lines of constant 𝜉 , may 
not  be  normal  to  𝐞̂1  and  𝐞̂3.    The  lamina  coordinate  system  rotates  rigidly  with  the 
element. 
The  transformation  of  vectors  from  the  global  to  lamina  coordinate  system  can 
now be defined in terms of the lamina basis vectors as 
⎧𝐴̂𝑥
⎫
}}
{{
𝐴̂𝑦
⎬
⎨
}}
{{
𝐴̂𝑧⎭
⎩
𝑒3𝑥
𝑒2𝑥
𝑒1𝑥
⎥⎤
⎢⎡
𝑒1𝑦    𝑒2𝑦    𝑒3𝑦
𝑒3𝑧 ⎦
𝑒2𝑧
𝑒1𝑧
⎣
{⎧𝐴𝑥
}⎫
𝐴𝑦
𝐴𝑧⎭}⎬
⎩{⎨
𝐀̂ =
=
= 𝐪𝐀, 
(13.35)
LS-DYNA Theory Manual 
Hughes-Liu Shell 
where 𝑒𝑖𝑥, 𝑒𝑖𝑦, 𝑒𝑖𝑧 are the global components of the lamina coordinate unit vectors; 𝐀̂ is a 
vector  in  the  lamina  coordinates,  and  𝐴  is  the  same  vector  in  the  global  coordinate 
system. 
13.3  Strains and Stress Update 
13.3.1  Incremental Strain and Spin Tensors 
The strain and spin increments are calculated from the incremental displacement 
gradient 
𝐺𝑖𝑗 =
∂Δ𝑢𝑖
∂𝑦𝑗
,
(13.36)
where Δ𝑢𝑖 are the incremental displacements and 𝑦𝑗 are the deformed coordinates.  The 
incremental strain and spin tensors are defined as the symmetric and skew-symmetric 
parts, respectively, of 𝐺𝑖𝑗: 
Δ𝜀𝑖𝑗 =
Δ𝜔𝑖𝑗 =
(𝐺𝑖𝑗 + 𝐺𝑗𝑖),
(𝐺𝑖𝑗 − 𝐺𝑗𝑖).
(13.37)
(13.38)
The  incremental  spin  tensor  Δ𝜔𝑖𝑗  is  used  as  an  approximation  to  the  rotational 
contribution of the Jaumann rate of the stress tensor; LS-DYNA implicit uses the more 
accurate Hughes-Winget transformation matrix (Equation (13.27)) with the incremental 
spin tensor for the rotational update.  The Jaumann rate update is approximated as: 
𝑛+1 = 𝜎𝑖𝑗
𝜎𝑖𝑗
𝑛 + 𝜎𝑖𝑝
𝑛 Δ𝜔𝑝𝑗 + 𝜎𝑗𝑝
𝑛 Δ𝜔𝑝𝑖,
(13.39)
where  the  superscripts  on  the  stress  refer  to  the  updated  (𝑛 + 1)  and  reference  (𝑛) 
configurations.    The  Jaumann  rate  update  of  the  stress  tensor  is  applied  in  the  global 
configuration before the constitutive evaluation is performed.  In the Hughes-Liu shell 
the stresses and history variables are stored in the global coordinate system. 
13.3.2  Stress Update 
To  evaluate  the  constitutive  relation,  the  stresses  and  strain  increments  are 
rotated  from  the  global  to  the  lamina  coordinate  system  using  the  transformation 
defined previously in Equation (13.35), viz. 
𝑙𝑛+1
𝜎𝑖𝑗
= 𝑞𝑖𝑘𝜎𝑘𝑛
𝑛+1𝑞𝑗𝑛,
 𝑙𝑛+1
2⁄
Δ𝜀𝑖𝑗
𝑛+1
= 𝑞𝑖𝑘Δ𝜀𝑘𝑛
2⁄
𝑞𝑗𝑛,
(13.40)
(13.41)
Hughes-Liu Shell 
LS-DYNA Theory Manual 
where the superscript 𝑙 indicates components in the lamina (local) coordinate system. 
The stress is updated incrementally: 
𝑙𝑛+1
𝜎𝑖𝑗
𝑙𝑛+1
= 𝜎𝑖𝑗
𝑙𝑛+1
2⁄
+ Δ𝜎𝑖𝑗
,
and rotated back to the global system: 
𝑙𝑛+1
𝑛+1 = 𝑞𝑘𝑖𝜎𝑘𝑛
𝜎𝑖𝑗
𝑞𝑛𝑗,
before computing the internal force vector. 
13.3.3  Incremental Strain-Displacement Relations 
The global stresses are now used to update the internal force vector 
int = ∫ 𝐓𝑎
𝐟𝑎
T𝐁𝑎
T𝛔𝑑𝜐,
(13.42)
(13.43)
(13.44)
int are the internal forces at node 𝑎, 𝐁𝑎 is the strain-displacement  matrix in the 
where 𝐟𝑎
lamina  coordinate  system  associated  with  the  displacements  at  node  𝑎,  and  𝐓𝑎  is  the 
transformation  matrix  relating  the  global  and  lamina  components  of  the  strain-
displacement matrix.  Because the B matrix relates six strain components to twenty-four 
displacements (six degrees of freedom at four nodes), it is convenient to partition the B 
matrix into four groups of six: 
Each 𝐁𝑎 submatrix is further partitioned into a portion due to strain and spin: 
𝐁 = [𝐁1 𝐁2 𝐁3 𝐁4],
𝐁𝑎 = [
𝐁𝑎
𝜔],
𝐁𝑎
𝜀 =
𝐁𝑎
𝐵1
⎡
𝐵2
⎢
⎢
𝐵̅̅̅̅2 𝐵̅̅̅̅1
⎢
⎢
⎢
𝐵̅̅̅̅3
⎣
𝐵̅̅̅̅3 𝐵̅̅̅̅2
𝐵4
𝐵5
𝐵̅̅̅̅5 𝐵̅̅̅̅4
𝐵̅̅̅̅1 𝐵̅̅̅̅6
⎤
⎥
⎥
, 
⎥
⎥
𝐵̅̅̅̅6 𝐵̅̅̅̅5
⎥
𝐵̅̅̅̅4⎦
𝜔 =
𝐁𝑎
where 
𝐵̅̅̅̅2 −𝐵̅̅̅̅1
⎡
⎢⎢
−𝐵̅̅̅̅3
⎣
𝐵̅̅̅̅3 −𝐵̅̅̅̅2
𝐵̅̅̅̅5 −𝐵̅̅̅̅4
𝐵̅̅̅̅1 −𝐵̅̅̅̅6
⎤
𝐵̅̅̅̅6 −𝐵̅̅̅̅5
, 
⎥⎥
𝐵̅̅̅̅4 ⎦
𝐵𝑖 =
⎧
{{{
⎨
{{{
⎩
𝑁𝑎,𝑖 =
(𝑁𝑎𝑧𝑎),𝑖−3 =
∂𝑁𝑎
∂𝑦𝑖
∂(𝑁𝑎𝑧𝑎)
∂𝑦𝑖−3
for 𝑖 = 1, 2, 3
. 
for 𝑖 = 4, 5, 6
(13.45)
(13.46)
(13.47)
(13.48)
(13.49)
Notes on strain-displacement relations:
LS-DYNA Theory Manual 
Hughes-Liu Shell 
•  The  derivatives  of  the  shape  functions  are  taken  with  respect  to  the  lamina 
coordinate system, e.g.,𝑦 = 𝑞𝑦. 
•  The superscript bar indicates the 𝐵’s are evaluated at the center of the lamina (0,
0, 𝜁 ).    The  strain-displacement  matrix  uses  the  ‘B-Bar’  (𝐵̅̅̅̅)approach  advocated 
by  Hughes  [1980].    In  the  NIKE3D  and  DYNA3D  implementations,  this  entails 
replacing certain rows of the B matrix and the strain increments with their coun-
terparts  evaluated  at  the  center  of  the  element.    In  particular,  the  strain-
displacement matrix is modified to produce constant shear and spin increments 
throughout the lamina. 
•  The resulting B-matrix is a 8 × 24 matrix.  Although there are six strain and three 
rotations increments, the B matrix has been modified to account for the fact that 
𝜎33 will be zero in the integration of Equation (13.44). 
13.4  Element Mass Matrix  
Hughes, Liu, and Levit [Hughes et al., 1981] describe the procedure used to form 
the shell element mass matrix in problems involving explicit transient dynamics.  Their 
procedure,  which  scales  the  rotary  mass  terms,  is  used  for  all  shell  elements  in  LS-
DYNA  including  those  formulated  by  Belytschko  and  his  co-workers.    This  scaling 
permits large critical time step sizes without loss of stability. 
The consistent mass matrix is defined by 
𝐌 = ∫ 𝜌𝐍T𝐍 𝑑𝜐𝑚
𝜐𝑚
,
(13.50)
but  cannot  be  used  effectively  in  explicit  calculations  where  matrix  inversions  are  not 
feasible.    In  LS-DYNA  only  three  and  four-node  shell  elements  are  used  with  linear 
interpolation  functions;  consequently,  we  compute  the  translational  masses  from  the 
consistent mass matrix by row summing, leading to the following mass at element node 
a: 
𝑀disp𝑎 = ∫ 𝜌𝜙𝑎 𝑑𝜐
.
(13.51)
The rotational masses are computed by scaling the translational mass at the node by the 
factor 𝛼: 
𝑀rot𝑎 = ∝ 𝑀disp𝑎,
∝ = max{∝1, ∝2},
∝1= ⟨𝑧𝑎⟩2 +
12
[𝑧𝑎]2,
∝2=
8ℎ
,
(13.52)
(13.53)
(13.54)
(13.55)
Hughes-Liu Shell 
LS-DYNA Theory Manual 
⟨𝑧𝑎⟩ =
(𝑧𝑎
+ + 𝑧𝑎
−)
,
[𝑧𝑎] = 𝑧𝑎
−.
+ − 𝑧𝑎
(13.56)
(13.57)
13.5  Accounting for Thickness Changes 
Hughes  and  Carnoy  [1981]  describe  the  procedure  used  to  update  the  shell 
thickness  due  to  large  membrane  stretching.    Their  procedure  with  any  necessary 
modifications is used across all shell element types in LS-DYNA.  One key to updating 
the thickness is an accurate calculation of the normal strain component Δ𝜀33.  This strain 
component is easily obtained for elastic materials but can require an iterative algorithm 
for  nonlinear  material  behavior.    In  LS-DYNA  we  therefore  default  to  an  iterative 
plasticity update to accurately determine Δ𝜀33. 
Hughes and Carnoy integrate the strain tensor through the thickness of the shell 
in order to determine a mean value Δ𝜀̅𝑖𝑗: 
Δ𝜀̅𝑖𝑗 =
∫ Δ𝜀𝑖𝑗
−1
𝑑𝜁 ,
and then project it to determine the straining in the fiber direction: 
𝛆̅ 𝑓 = 𝐘̂TΔ𝛆̅𝐘̂.
(13.58)
(13.59)
Using the interpolation functions through the integration points the strains in the fiber 
directions are extrapolated to the nodal points if 2 × 2 selectively reduced integration is 
employed.  The nodal fiber lengths can now be updated: 
𝑛+1 = ℎ𝑎
ℎ𝑎
𝑛 (1 + 𝜀̅𝑎
𝑓 ).
(13.60)
13.6  Fully Integrated Hughes-Liu Shells 
It  is  well  known  that  one-point  integration  results  in  zero  energy  modes  that 
must be resisted.  The four-node under integrated shell with six degrees of freedom per 
node  has  nine  zero  energy  modes,  six  rigid  body  modes,  and  four  unconstrained 
drilling  degrees  of  freedom.    Deformations  in  the  zero  energy  modes  are  always 
troublesome  but  usually  not  a  serious  problem  except  in  regions  where  boundary 
conditions such as point loads are active.  In areas where the zero energy modes are a 
problem, it is highly desirable to provide the option of using the original formulation of 
Hughes-Liu with selectively reduced integration.
LS-DYNA Theory Manual 
Hughes-Liu Shell 
Figure 13.5.  Selectively reduced integration rule results in four inplane points
being used. 
The major disadvantages of full integration are two-fold: 
nearly four times as much data must be stored; 
the  operation  count  increases  three-  to  fourfold.    The  level  3  loop is  added  as 
shown in Figure 13.6 
1. 
2. 
However, these disadvantages can be more than offset by the increased reliability and 
accuracy. 
We  have  implemented  two  version  of  the  Hughes-Liu  shell  with  selectively 
reduced  integration.    The  first  closely  follows  the  intent  of  the  original  paper,  and 
therefore  no  assumptions  are  made  to  reduce  costs,  which  are  outlined  in  operation 
counts in Table 10.1.  These operation counts can be compared with those in Table 10.2 
for the Hughes-Liu shell with uniformly reduced integration.  The second formulation, 
which reduces the number of operation by more than a factor of two, is referred to as 
the  co-rotational  Hughes-Liu  shell  in  the  LS-DYNA  user’s  manual.    This  shell  is 
considerably cheaper due to the following simplifications: 
•  Strains rates are not centered.  The strain displacement matrix is only computed 
at time 𝑛 + 1 and not at time 𝑛 + 1 ⁄ 2. 
•  The  stresses  are  stored  in  the  local  shell  system  following  the  Belytschko-Tsay 
shell.    The  transformations  of  the  stresses  between  the  local  and  global  coordi-
nate systems are thus avoided. 
•  The  Jaumann  rate  rotation  is  not  performed,  thereby  avoiding  even  more 
computations.    This  does  not  necessarily  preclude  the  use  of  the  shell  in  large 
deformations. 
•  To  study  the  effects  of  these  simplifying  assumptions,  we  can  compare  results 
with those obtained with the full Hughes-Liu shell.  Thus far, we have been able 
to get comparable results.
Hughes-Liu Shell 
LS-DYNA Theory Manual 
LEVEL L1 - Do over each element group
                      gather data, midstep geometry calculation
LEVEL 2 - For each thickness integration point
                   center of element calculations for selective
                   reduced integration
LEVEL 3 - Do over 4 Gauss points
                   stress update and force
                   contributions
LEVEL 2 - Completion
LEVEL L1 - Completion
Figure 13.6.  An inner loop, LEVEL 3, is added for the Hughes-Liu shell with 
selectively reduced integration. 
LEVEL L1 - Once per element 
Midstep translation geometry, etc. 
Midstep calculation of 𝑌̂  318 
204 
LEVEL L2 - For each integration point through thickness (NT points) 
Strain increment at (0, 0, 𝜁 ) 316 
Hughes-Winget rotation matrix  33 
Square root of Hughes-Winget matrix 
Rotate strain increments into lamina coordinates 
Calculate rows 3-8 of B matrix 
919 
47 
66 
LEVEL L3 - For each integration point in lamina 
Rotate stress to n+1/2 configuration 
75 
Incremental displacement gradient matrix 
Rotate stress to lamina system 
Rotate strain increments to lamina system 
Constitutive model  model dependent 
Rotate stress back to global system 
Rotate stress to n+1 configuration 75 
Calculate rows 1 and 2 of B matrix 
Stresses in n+1 lamina system 
Stress divergence 
245 
75 
75 
69 
358 
370 
55
LS-DYNA Theory Manual 
Hughes-Liu Shell 
TOTAL 
522 +NT {1381 +4 * 1397} 
Table 10.1.  Operation counts for the Hughes-Liu shell with selectively reduced 
integration. 
LEVEL L1 - Once per element 
Calculate displacement increments 
Element areas for time step 
Calculate 𝑌̂  238 
53 
24 
LEVEL L2 and L3 - Integration point through thickness (NT points) 
284 
Incremental displacement gradient matrix 
Jaumann rotation for stress 33 
Rotate stress into lamina coordinates 
Rotate stain increments into lamina coordinates 
Constitutive model  model dependent 
Rotate stress to n+1 global coordinates  69 
125 
Stress divergence 
75 
81 
LEVEL L1 - Cleanup 
Finish stress divergence 
Hourglass control  356 
60 
TOTAL   
731 +NT * 667 
Table 10.2.  Operation counts for the LS-DYNA implementation of the uniformly 
reduced 
Hughes-Liu shell.
LS-DYNA Theory Manual 
Transverse Shear Treatment For Layered Shell 
14    
Transverse Shear Treatment For 
Layered Shell 
The  shell  element  formulations  that  include  the  transverse  shear  strain 
components are based on the first order shear deformation theory, which yield constant 
through thickness transverse shear strains.  This violates the condition of zero traction 
on the top and bottom surfaces of the shell.  Normally, this is corrected by the use of a 
shear  correction  factor.    The  shear  correction  factor  is  5/6  for  isotropic  materials; 
however, this value is incorrect for sandwich and laminated shells.  Not accounting for 
the  correct  transverse  shear  strain  and  stress  could  yield  a  very  stiff  behavior  in 
sandwich  and  laminated  shells.    This  problem  is  addressed  here  by  the  use  of  the 
equilibrium equations without gradient in the y-direction as described by what follows.  
Consider the stresses in a layered shell: 
(𝑖)(𝜀𝑥
(𝑖) = 𝐶11
𝜎𝑥
(𝑖)𝜀𝑥
(𝑖) = 𝐶12
𝜎𝑦
(𝑖)(𝜀𝑥𝑦
(𝑖) = 𝐶44
𝜏𝑥𝑦
∘ + 𝑧𝜒𝑥) + 𝐶12
(𝑖)𝜀𝑦
∘ + 𝐶22
∘ + 𝑧(𝐶12
∘ + 𝑧𝜒𝑥𝑦). 
(𝑖)(𝜀𝑦
(𝑖)𝜒𝑥 + 𝐶22
∘ + 𝑧𝜒𝑦) = 𝐶11
(𝑖)𝜒𝑦, 
(𝑖)𝜀𝑥
∘ + 𝐶12
(𝑖)𝜀𝑦
∘ + 𝑧(𝐶11
(𝑖)𝜒𝑥 + 𝐶12
(𝑖)𝜒𝑦), 
Assume that the bending center 𝑧̅𝑥 is known.  Then 
(𝑖)𝜒𝑦) + 𝐶11
(𝑖) = (𝑧 − 𝑧̅𝑥)(𝐶11
𝜎𝑥
(𝑖)𝜒𝜒 + 𝐶12
(𝑖)𝜀𝑥(𝑧̅𝑥) + 𝐶12
(𝑖)𝜀𝑦(𝑧̅𝑥). 
The bending moment is given by the following equation: 
𝑁𝐿
⎜⎛∑ 𝐶11
⎝
𝑖=1
𝑧𝑖
𝑧𝑖−1
(𝑖) ∫ (𝑧 − 𝑧̅𝑥)2
𝑀𝑥𝑥 = 𝜒𝑥
or 
𝑁𝐿
𝑑𝑧
⎟⎞ + 𝜒𝑦
⎠
⎜⎛∑ 𝐶12
⎝
𝑖=1
𝑧𝑖
𝑧𝑖−1
(𝑖) ∫ (𝑧 − 𝑧̅𝑥)2
𝑑𝑧
⎟⎞ 
⎠
𝑀𝑥𝑥 =
𝑁𝐿
[𝜒𝑥 ∑ 𝐶11
(𝑖)[(𝑧𝑖
𝑖=1
3 − 𝑧𝑖−1
3 ) − (𝑧𝑖 − 𝑧𝑖−1)𝑧̅𝑥
2]
      + 𝜒𝑦 ∑ 𝐶12
(𝑖)[(𝑧𝑖
3 − 𝑧𝑖−1
3 ) − (𝑧𝑖 − 𝑧𝑖−1)𝑧̅𝑥
2]
] 
𝑁𝐿
𝑖=1
(14.1)
(14.2)
(14.3)
(14.4)
Transverse Shear Treatment For Layered Shell 
LS-DYNA Theory Manual 
where “𝑁𝐿” is the number of layers in the material. 
Assume 𝜀𝑦 = 0 and 𝜎𝑥 = 𝐸𝜒𝜀𝜒, let 
𝑁𝐿
(𝐸𝐼)𝑥 = ∑
𝑖=1
(𝑖)[(𝑧𝑖
𝐸𝑥
3 − 𝑧𝑖−1
3 ) − (𝑧𝑖 − 𝑧𝑖−1)𝑧̅𝑥
2],
then 
and 
𝜀𝑥 =
𝑧 − 𝑧̅𝑥
= (𝑧 − 𝑧̅𝑥)𝜒𝑥,
𝑀𝑥𝑥 =
(𝜒𝑥(𝐸𝐼)𝑥),
𝜒𝑥 =
3𝑀𝑥𝑥
(𝐸𝐼)𝑥
.
Therefore, the stress becomes 
(𝑖) =
𝜎𝑥
3𝑀𝑥𝑥𝐸𝑥
(𝑖)(𝑧 − 𝑧̅𝑥)
(𝐸𝐼)𝑥
.
Now considering the first equilibrium equation, one can write the following: 
∂𝜏𝑥𝑧
∂𝑧
= −
∂𝜎𝑥
∂𝑥
= −
3𝑄𝑥𝑧𝐸𝑥
(𝑗)(𝑧 − 𝑧̅𝑥)
,
(𝐸𝐼)𝑥
(𝑗) = −
𝜏𝑥𝑧
3𝑄𝑥𝑧𝐸𝑥
(𝑗) (𝑧2
(𝐸𝐼)𝑥
− 𝑧𝑧̅𝑥)
+ 𝐶𝑗, 
(14.5)
(14.6)
(14.7)
(14.8)
(14.9)
(14.10)
(14.11)
where  𝑄𝑥𝑧  is  the  shear  force  and  𝐶𝑗  is  the  constant  of  integration.    This  constant  is 
obtained from the transverse shear stress continuity requirement at the interface of each 
layer.  Let 
then 
𝑄𝑥𝑧𝐸𝑥
(𝑖) (
𝑧𝑖−1
− 𝑧𝑖−1𝑧̅𝑥)
(𝐸𝐼)𝑥
𝐶𝑗 =
+ 𝜏𝑥𝑧
𝑖−1,
and 
(𝑖) = 𝜏𝑥𝑧
𝜏𝑥𝑧
(𝑖−1) +
(𝑖)
𝑄𝑥𝑧𝐸𝑥
(𝐸𝐼)𝑥
𝑧𝑖−1
[
− 𝑧𝑖−1𝑧̅𝑥 −
𝑧2
+ 𝑧𝑧̅𝑥].
For the first layer 
(14.12)
(14.13)
LS-DYNA Theory Manual 
Transverse Shear Treatment For Layered Shell 
𝜏𝑥𝑧 = −
(1)
3𝑄𝑥𝑧𝐶11
(𝐸𝐼)𝑥
𝑧2 − 𝑧𝑜
[
− 𝑧̅𝑥(𝑧 − 𝑧𝑜)],
(14.14)
for subsequent layers 
𝜏𝑥𝑧 = 𝜏𝑥𝑧
(𝑖−1) −
(𝑖)
3𝑄𝑥𝑧𝐶11
(𝐸𝐼)𝑥
𝑧2 − 𝑧𝑖−1
[
− 𝑧̅𝑥(𝑧 − 𝑧𝑖−1)] ,
𝑧𝑖−1 ≤ 𝑧 ≤ 𝑧𝑖. 
(14.15)
(𝑖−1)  is  the  stress  in  previous  layer  at  the  interface  with  the  current  layer.    The 
Here  𝜏𝑥𝑧
shear stress can also be expressed as follows: 
𝜏𝑥𝑧 = −
(𝑖)
3𝑄𝑥𝑧𝐶11
(𝐸𝐼)𝑥
(𝑖) +
[𝑓𝑥
𝑧2 − 𝑧𝑖−1
− 𝑧̅𝑥(𝑧 − 𝑧𝑖−1)],
(14.16)
where 
and 
(𝑖) =
𝑓𝑥
𝑖−1
(𝑖) ∑ 𝐶11
𝐶11
𝑗=1
(𝑗)ℎ𝑗 [
𝑧𝑗 + 𝑧𝑗+1
− 𝑧̅𝑥]
,
ℎ𝑗 = 𝑧𝑗 − 𝑧𝑗−1.
(14.17)
(14.18)
To  find  𝑄𝑥𝑧,  the  shear  force,  assume  that  the  strain  energy  expressed  through 
average shear modules, 𝐶̅66, is equal to the strain energy expressed through the derived 
expressions as follows: 
𝑈 =
𝑄𝑥𝑧
𝐶̅66ℎ
=
∫
𝜏𝑥𝑧
𝐶66
𝑑𝑧,
2 ∫
𝐶11
𝐶66
(𝑖) +
[𝑓𝑥
2 )
(𝑧2 − 𝑧𝑖−1
− 𝑧̅𝑥(𝑧 − 𝑧𝑖−1)]
𝑑𝑧 
9ℎ
(𝐸𝐼)𝑥
9ℎ
(𝐸𝐼)𝑥
60
𝐶̅66
=
=
=
then 
9ℎ
(𝑖) +
𝑁𝐿
2 ∑
𝑖=1
[𝑓𝑥
𝑧𝑖
∫
𝑧𝑖−1
(𝑖))2
(𝐶11
(𝑖)
𝐶66
(𝑖))2ℎ
(𝐶11
𝐶66
+ 𝑧̅𝑥ℎ𝑖[20𝑧̅𝑥ℎ𝑖 + 35𝑧𝑖−1
2 ) + 8𝑧𝑖−1
− 7𝑧𝑖−1
𝑁𝐿
2 ∑
𝑖[60𝑓𝑥
4 }, 
{𝑓𝑥
(𝐸𝐼)𝑥
𝑧2 − 𝑧𝑖−1
− 𝑧̅𝑥(𝑧 − 𝑧𝑖−1)]
𝑑𝑧 
𝑖 + 20ℎ𝑖(𝑧𝑖 + 2𝑧𝑖−1 − 3𝑧̅𝑥)]
2 − 10𝑧𝑖−1(𝑧𝑖 + 𝑧𝑖−1) − 15𝑧𝑖
2] + 𝑧𝑖(𝑧𝑖 + 𝑧𝑖−1)(3𝑧𝑖
𝑄𝑥𝑧 = 𝜏̅𝑥𝑧ℎ = 𝐶̅66𝛾̅̅̅̅𝑥𝑧ℎ,
to calculate 𝑧̅𝑥 use 𝜏𝑥𝑧 for last layer at surface 𝑧 = 0, 
𝑁𝐿
(𝑖)
∑ 𝐶11
𝑖=1
[(
2 − 𝑧𝑖−1
𝑧𝑖
) − 𝑧̅𝑥(𝑧𝑖 − 𝑧𝑖−1)] = 0,
(14.19)
(14.20)
(14.21)
(14.22)
Transverse Shear Treatment For Layered Shell 
LS-DYNA Theory Manual 
where 
Algorithm: 
𝑧̅𝑥 =
𝑁𝐿
∑ 𝐶11
𝑖=1
(𝑖)ℎ𝑖(𝑧𝑖 + 𝑧𝑖+1)
. 
𝑁𝐿
(𝑖)ℎ𝑖
2 ∑ 𝐶11
𝑖=1
(14.23)
The  following  algorithm  is  used  in  the  implementation  of  the  transverse  shear 
treatment. 
1.  Calculate 𝑧̅𝑥 according to equation (14.23) 
2.  Calculate 𝑓𝑥
𝑖 according to equation (14.17) 
3.  Calculate 1
𝑁𝐿
(𝑖)
3 ∑ 𝐶11
𝑖=1
(𝑧𝑖
3 − 𝑧𝑖−1
3 ) 
4.  Calculate ℎ[1
𝑁𝐿
(𝑖)
3 ∑ 𝐶11
𝑖=1
3 − 𝑧𝑖−1
3 )]
(𝑧𝑖
5.  Calculate 𝐶̅66 according to equation (14.20) 
6.  Calculate 𝑄𝑥𝑧 = 𝐶̅66𝛾̅̅̅̅𝑥𝑧ℎ 
7.  Calculate 𝜏𝑥𝑧 according to equation (14.16) 
Steps  1-5  are  performed  at  the  initialization  stage.    Step  6  is  performed  in  the  shell 
formulation  subroutine,  and  step  7  is  performed  in  the  stress  calculation  inside  the 
constitutive subroutine.
LS-DYNA Theory Manual 
Eight-Node Solid Shell Element 
15    
Eight-Node Solid Shell Element 
The  isoparametric  eight-node  brick  element  discussed  in  Section  3  forms  the 
basis  for  tshell  formulation  1,  a  solid  shell  element  with  enhancements  based  on  the 
Hughes-Liu  and  the  Belytschko-Lin-Tsay  shells.    Like  the  eight-node  brick,  the 
geometry is interpolated from the nodal point coordinates as: 
𝑥𝑖(𝑋𝛼, 𝑡) = 𝑥𝑖(𝑋𝛼(𝜉 , 𝜂, 𝜁 ), 𝑡) = ∑ 𝜙𝑗
𝑗=1
(𝜉 , 𝜂, 𝜁 )𝑥𝑖
𝑗(𝑡),
𝜙𝑗 =
(1 + 𝜉 𝜉𝑗)(1 + 𝜂𝜂𝑗)(1 + 𝜁 𝜁𝑗).
As with solid elements, 𝐍 is the 3 × 24 rectangular interpolation matrix: 
𝐍(𝜉 , 𝜂, 𝜁 ) =
𝜑1
⎡
⎢
⎣
𝜑1
𝜑1
𝜑2
0 … 0
𝜑2 … 𝜑8
0 … 0
⎤
, 
⎥
𝜑8⎦
𝛔 is the stress vector: 
and 𝐁 is the 6 × 24 strain-displacement matrix: 
𝛔T = (𝜎𝑥𝑥, 𝜎𝑦𝑦, 𝜎𝑧𝑧, 𝜎𝑥𝑦, 𝜎𝑦𝑧, 𝜎𝑧𝑥),
(15.1)
(15.2)
(15.3)
(15.4)
Eight-Node Solid Shell Element 
LS-DYNA Theory Manual 
Upper shell surface. The numbering of
the solid shell determines its orientation
Node
-1
-1
-1
-1
-1
-1
-1
-1
-1
-1
-1
-1
Figure 15.1.  Eight node solid shell element 
𝐁 =
∂
∂𝑥
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
∂
∂𝑦
∂
∂𝑧
∂
∂𝑦
∂
∂𝑥
∂
∂𝑧
∂
∂𝑧
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
∂
⎥
⎥
∂𝑦
⎥
∂
⎥
∂𝑥⎦
𝐍, 
(15.5)
Terms in the strain-displacement matrix are readily calculated.  Note that 
∂𝜑𝑖
∂𝜉
∂𝜑𝑖
∂𝜂
∂𝜑𝑖
∂𝜁
=
=
=
∂𝜑𝑖
∂𝑥
∂𝜑𝑖
∂𝑥
∂𝜑𝑖
∂𝑥
∂𝑥
∂𝜉
∂𝑥
∂𝜂
∂𝑥
∂𝜁
+
+
+
∂𝜑𝑖
∂𝑦
∂𝜑𝑖
∂𝑦
∂𝜑𝑖
∂𝑦
∂𝑦
∂𝜉
∂𝑦
∂𝜂
∂𝑦
∂𝜁
+
+
+
∂𝜑𝑖
∂𝑧
∂𝜑𝑖
∂𝑧
∂𝜑𝑖
∂𝑧
∂𝑧
∂𝜉
∂𝑧
∂𝜂
∂𝑧
∂𝜁
,
, 
,
(15.6)
which can be rewritten as
LS-DYNA Theory Manual 
Eight-Node Solid Shell Element 
∂𝜑𝑖
⎤
⎡
∂𝜉
⎥
⎢
⎥
⎢
∂𝜑𝑖
⎥
⎢
⎥
⎢
∂𝜂
⎥
⎢
⎥
⎢
∂𝜑𝑖
⎥
⎢
∂𝜁 ⎦
⎣
=
∂𝑥
∂𝜉
∂𝑥
∂𝜂
∂𝑥
∂𝜁
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
∂𝑦
∂𝜉
∂𝑦
∂𝜂
∂𝑦
∂𝜁
∂𝑧
⎤
∂𝜉
⎥
⎥
∂𝑧
⎥
⎥
∂𝜂
⎥
⎥
∂𝑧
⎥
∂𝜁 ⎦
∂𝜑𝑖
⎤
⎡
∂𝑥
⎥
⎢
⎥
⎢
∂𝜑𝑖
⎥
⎢
⎥
⎢
∂𝑦
⎥
⎢
∂𝜑𝑖
⎥
⎢
∂𝑧 ⎦
⎣
= 𝐉
∂𝜑𝑖
⎤
∂𝑥
⎥
⎥
∂𝜑𝑖
⎥
. 
⎥
∂𝑦
⎥
∂𝜑𝑖
⎥
∂𝑧 ⎦
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎣
Inverting the Jacobian matrix, 𝐉, we can solve for the desired terms 
∂𝜑𝑖
⎤
⎡
∂𝑥
⎥
⎢
⎥
⎢
∂𝜑𝑖
⎥
⎢
⎥
⎢
∂𝑦
⎥
⎢
∂𝜑𝑖
⎥
⎢
∂𝑧 ⎦
⎣
= 𝐉−1
∂𝜑𝑖
⎤
⎡
∂𝜉
⎥
⎢
⎥
⎢
∂𝜑𝑖
⎥
⎢
⎥
⎢
∂𝜂
⎥
⎢
⎥
⎢
∂𝜑𝑖
⎥
⎢
∂𝜁 ⎦
⎣
. 
(15.7)
(15.8)
To  obtain  shell-like  behavior  from  the  solid  element,  it  is  necessary  to  use 
multiple integration points through the shell thickness along the 𝜁  axis while employing 
a  plane  stress  constitutive  subroutine.    Consequently,  it  is  necessary  to  construct  a 
reference  surface  within  the  brick  shell.    We  locate  the  reference  surface  midway 
between the upper and lower surfaces and  construct a local coordinate system exactly 
as  was  done  for  the  Belytschko-Lin-Tsay  shell  element.    Following  the  procedure 
outlined  in  Section  7,  Equations  (7.1)  –  (7.3),  the  local  coordinate  system  can  be 
constructed as depicted in Figure 15.2.  Equation (7.5a) gives the transformation matrix 
in terms of the local basis: 
{𝐀} =
{⎧𝐴𝑥
}⎫
𝐴𝑦
𝐴𝑧⎭}⎬
⎩{⎨
=
𝑒3𝑥
𝑒1𝑥    𝑒2𝑥
⎥⎤
⎢⎡
𝑒1𝑦    𝑒2𝑦    𝑒3𝑦
𝑒3𝑧 ⎦
𝑒1𝑧    𝑒2𝑧
⎣
⎧𝐴̂𝑥
⎫
}}
{{
𝐴̂𝑦
⎬
⎨
}}
{{
𝐴̂𝑧⎭
⎩
= [𝛍]{𝐀̂} = [𝐪]T{𝐀̂}. 
(15.9)
As  with  the  Hughes-Liu  shell,  the  next  step  is  to  perform  the  Jaumann  rate 
update: 
𝑛+1 = 𝜎𝑖𝑗
𝜎𝑖𝑗
𝑛 + 𝜎𝑖𝑝
𝑛 Δ𝜔𝑝𝑗 + 𝜎𝑗𝑝
𝑛 Δ𝜔𝑝𝑖,
(15.10)
to account for the material rotation between time steps 𝑛 and 𝑛 + 1.  The Jaumann rate 
update of the stress tensor is applied in the global configuration before the constitutive 
evaluation is performed.  In the solid shell, as in the Hughes-Liu shell, the stresses and 
history  variables  are  stored  in  the  global  coordinate  system.    To  evaluate  the 
constitutive relation, the stresses and the strain increments are rotated from the global 
to the lamina coordinate system using the transformation defined previously:  
𝑙𝑛+1
𝜎𝑖𝑗
= 𝑞𝑖𝑘𝜎𝑘𝑛
𝑛+1𝑞𝑗𝑛,
 𝑙𝑛+1
2⁄
Δ𝜀𝑖𝑗
𝑛+1
= 𝑞𝑖𝑘Δ𝜀𝑘𝑛
2⁄
𝑞𝑗𝑛,
(15.11)
(15.12)
Eight-Node Solid Shell Element 
LS-DYNA Theory Manual 
A reference surface is constructed within
the solid shell element and the local reference
system is defined. 
y^
e^
s3
e^
r42
r31
e^
s1
x^
r21
  Figure 15.2.  Construction of the reference surface in the solid shell element. 
where  the  superscript  l  indicates  components  in  the  lamina  (local)  coordinate  system.  
The stress is updated incrementally: 
𝑙𝑛+1
𝜎𝑖𝑗
𝑙𝑛+1
= 𝜎𝑖𝑗
𝑙𝑛+1
2⁄
+ Δ𝜎𝑖𝑗
.
Independently from the constitutive evaluation  
𝑙 = 0,
𝜎33
(15.13)
(15.14)
which  ensures  that  the  plane  stress  condition  is  satisfied,  we  update  the  normal  stress 
which is used as a penalty to maintain the thickness of the shell: 
penalty)
(𝜎33
n+1
= (𝜎33
penalty)
+ 𝐸Δ𝜀33
,
(15.15)
where 𝐸 is the elastic Young’s modulus for the material.  The stress tensor of Equation 
(15.13) is rotated back to the global system: 
𝑙 )
𝑛+1 = 𝑞𝑘𝑖(𝜎𝑘𝑛
𝜎𝑖𝑗
𝑛+1
𝑞𝑛𝑗.
(15.16)
A penalty stress tensor is then formed by transforming the normal penalty stress tensor 
(a null tensor except for the 33 term) back to the global system: 
n+1
penalty)
(𝜎𝑖𝑗
= 𝑞𝑘𝑖 [(𝜎𝑖𝑗
penalty)
𝑛+1
]
𝑞𝑛𝑗,
15-4 (Eight-Node Solid Shell Element)
LS-DYNA Theory Manual 
Eight-Node Solid Shell Element 
before  computing  the  internal  force  vector.    The  internal  force  vector  can  now  be 
computed: 
𝐟int = ∫(𝐁𝑛+1)
[𝝈𝑛+1 + (𝝈penalty)
𝑛+1
] 𝑑𝜐.
(15.18)
The brick shell exhibits no discernible locking problems with this approach.   
The treatment of the hourglass modes is identical to that described for the solid 
elements in Section 3.
LS-DYNA Theory Manual 
Eight-Node Solid Element for Thick Shell Simulations 
16    
Eight-Node Solid Element for Thick 
Shell Simulations 
16.1  Abstract 
Tshell formulation 3 is an eight-node hexahedral  element incorporated into LS-
DYNA  to  simulate  thick  shell  structures.    The  element  formulation  is  derived  in  a  co-
rotational  coordinate  system  and  the  strain  operator  is  calculated  with  a  Taylor  series 
expansion  about  the  center  of  the  element.    Special  treatments  are  made  on  the 
dilatational strain component and shear strain components to eliminate the volumetric 
and  shear  locking.    The  use  of  consistent  tangential  stiffness  and  geometric  stiffness 
greatly improves the convergence rate in implicit analysis. 
16.2  Introduction 
Large-scale  finite  element  analyses  are  extensively  used  in  engineering  designs 
and  process  controls.    For  example,  in  automobile  crashworthiness,  hundreds  of 
thousands of unknowns are involved in the computer simulation models, and in metal 
forming  processing,  tests  in  the  design  of  new  dies  or  new  products  are  done  by 
numerical computations instead of costly experiments.  The efficiency of the elements is 
of  crucial  importance  to  speed  up  the  design  processes  and  reduce  the  computational 
costs  for  these  problems.    Over  the  past  ten  years,  considerable  progress  has  been 
achieved in developing fast and reliable elements.   
In the simulation of shell structures, Belytschko-Lin-Tsay [Belytschko, 1984a] and 
Hughes-Liu  [Hughes,  1981a  and  1981b]  shell  elements  are  widely  used.    However,  in 
some  cases  thick  shell  elements  are  more  suitable.    For  example,  in  the  sheet  metal 
forming  with  large  curvature,  traditional  thin  shell  elements  cannot  give  satisfactory
Eight-Node Solid Element for Thick Shell Simulations 
LS-DYNA Theory Manual 
results.  Also thin shell elements cannot give us detailed strain information though the 
thickness.    In  LS-DYNA,  the  eight-node  solid  thick  shell  element  is  still  based  on  the 
Hughes-Liu  and  Belytschko-Lin-Tsay  shells  [Hallquist,  1998].    A  new  eight-node  solid 
element based on Liu, 1985, 1994 and 1998 is incorporated into LS-DYNA, intended for 
thick  shell  simulation.    The  strain  operator  of  this  element  is  derived  from  a  Taylor 
series  expansion  and  special  treatments  on  strain  components  are  utilized  to  avoid 
volumetric and shear locking.   
The  organization  of  this  paper  is  as  follows.    The  element  formulations  are 
described  in  the  next  section.    Several  numerical  problems  are  studied  in  the  third 
section, followed by the conclusions. 
16.3  Element Formulations 
16.3.1  Strain Operator 
The  new  element  is  based  on  the  eight-node  hexahedral  element  proposed  and 
enhanced  by  Liu,  1985,  1994,  1998.    For  an  eight-node  hexahedral  element,  the  spatial 
coordinates,  𝑥𝑖,  and  the  velocity  components,  𝑣𝑖,  in  the  element  are  approximated  in 
terms of nodal values, x𝑖aand v𝑖a, by 
𝑥𝑖 = ∑ 𝑁𝑎
𝑎=1
(𝜉 , 𝜂, 𝜁 )𝑥𝑖𝑎,
(16.1)
𝑣𝑖 = ∑ 𝑁𝑎
𝑎 = 1
(𝜉 , 𝜂, 𝜁 )𝑣𝑖𝑎,
𝑖 = 1, 2, 3,
𝑁𝑎(𝜉, 𝜂, 𝜁 ) =
(1 + 𝜉𝑎𝜉 )(1 + 𝜂𝑎𝜂)(1 + 𝜁𝑎𝜁 ),
(16.2)
(16.3)
and the subscripts 𝑖 and a denote coordinate components ranging from one to three and 
the  element  nodal  numbers  ranging  from  one  to  eight,  respectively.    The  referential 
coordinates 𝜉 , 𝜂, and 𝜁  of node a are denoted by 𝜉𝑎, 𝜂𝑎, and 𝜁𝑎, respectively. 
The strain rate (or rate of deformation), 𝛆̇, is composed of six components, 
and is related to the nodal velocities by a strain operator, 𝐁̅̅̅̅̅, 
𝛆̇T = [𝜀𝑥𝑥 𝜀𝑦𝑦 𝜀𝑧𝑧 𝜀𝑥𝑦 𝜀𝑦𝑧 𝜀𝑧𝑥],
𝛆̇ = 𝐁̅̅̅̅̅(𝜉 , 𝜂, 𝜁 )𝐯,
where 
𝐯T   = [vx1 vy1 vz1 ⋯ vx8 vy8 vz8],
(16.4)
(16.5)
(16.6)
LS-DYNA Theory Manual 
Eight-Node Solid Element for Thick Shell Simulations 
𝐁̅̅̅̅̅ =
B̅̅̅̅̅𝑥𝑥
⎤
⎡
B̅̅̅̅̅𝑦𝑦
⎥
⎢
⎥
⎢
B̅̅̅̅̅𝑧𝑧
⎥
⎢
⎥
⎢
B̅̅̅̅̅𝑥𝑦
⎥
⎢
⎥
⎢
⎥
⎢
B̅̅̅̅̅𝑦𝑧
⎥
⎢
B̅̅̅̅̅𝑧𝑥⎦
⎣
=
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎣
𝐵1(1)
𝐵2(1)
⋯ 𝐵1(8)
⋯
𝐵3(1) ⋯
𝐵2(1) 𝐵1(1)
⋯ 𝐵2(8) 𝐵1(8)
𝐵2(8)
⎤
⎥
⎥
𝐵3(8)
⎥
, 
⎥
⎥
𝐵3(8) 𝐵2(8)
⎥
𝐵1(8)⎦
𝐵3(1)
𝐵3(1) 𝐵2(1) ⋯
𝐵1(1) ⋯ 𝐵3(8)
B1
⎤ =
⎡
B2
⎥
⎢
B3⎦
⎣
𝑁,𝑥 (𝜉 , 𝜂, 𝜁 )
⎤
⎡
𝑁,𝑦 (𝜉 , 𝜂, 𝜁 )
. 
⎥⎥
⎢⎢
𝑁,𝑧 (𝜉 , 𝜂, 𝜁 )⎦
⎣
(16.7)
(16.8)
Unlike  standard  solid  element  where  the  strain  operator  is  computed  by 
differentiating the shape functions, the strain operator for this new element is expanded 
in  a  Taylor  series  about  the  element  center  up  to  bilinear  terms  as  follows  [Liu,  1994, 
1998], 
𝐁̅̅̅̅̅(𝜉 , 𝜂, 𝜁 )   =   𝐁̅̅̅̅̅(0) + 𝐁̅̅̅̅̅,𝜉 (0)𝛏 + 𝐁̅̅̅̅̅,𝜂 (0)𝛈 + 𝐁̅̅̅̅̅,𝜁 (0)𝛇
    + 𝐁̅̅̅̅̅,𝜉𝜂 (0)𝛏𝛈  +   𝐁̅̅̅̅̅,𝜂𝜁 (0)𝛈𝛇 + 𝐁̅̅̅̅̅,𝜁𝜉 (0)𝛇𝛏 .
Let 
T = 𝐱T = [𝑥1
𝐱1
𝑥2
𝑥3
𝑥4
𝑥5
𝑥6
𝑥7
𝑥8],
T = 𝐲T = [𝑦1
𝐱2
𝑦2
𝑦3
T = 𝐳T = [𝑧1
𝐱3
𝑧2
𝑧3
𝑦4
𝑧4
𝑦5
𝑦6
𝑦7
𝑦8],
𝑧5
𝑧6
𝑧7
𝑧8],
𝛏T   =   [−1
1 −1 −1
1 −1],
𝛈T   =   [−1 −1
1 −1 −1
1],
𝛇T   =   [−1 −1 −1 −1
the Jacobian matrix at the center of the element can be evaluated as 
1],
𝐉(0) = [J𝑖𝑗] =
𝛏T𝐲 𝛏T𝐳
𝛏T𝐱
⎤
⎡
𝛈T𝐱 𝛈T𝐲 𝛈T𝐳
⎥⎥
⎢⎢
𝛇T𝐲 𝛇T𝐳⎦
𝛇T𝐱
⎣
; 
(16.9)
(16.10)
(16.11)
(16.12)
(16.13)
(16.14)
(16.15)
(16.16)
the determinant of the Jacobian matrix is denoted by j0 and the inverse matrix of 𝐉(0) is 
denoted by 𝐃 
𝐃 = [D𝑖𝑗] = 𝐉−1(0).
(16.17)
The gradient vectors and their derivatives with respect to the natural coordinates 
at the center of the element are given as follows,
Eight-Node Solid Element for Thick Shell Simulations 
LS-DYNA Theory Manual 
𝐛1 = 𝐍,𝑥 (0) =
𝐛2 = 𝐍,𝑦 (0) =
𝐛3 = 𝐍,𝑧 (0) =
[𝐷11𝛏 + 𝐷12𝛈 + 𝐷13𝛇],
[𝐷21𝛏 + 𝐷22𝛈 + 𝐷23𝛇],
[𝐷31𝛏 + 𝐷32𝛈 + 𝐷33𝛇],
𝐛1,𝜉 = 𝐍,𝑥𝜉 (0) =
𝐛2,𝜉 = 𝐍,𝑦𝜉 (0) =
𝐛3,𝜉 = 𝐍,𝑧𝜉 (0) =
𝐛1,𝜂 = 𝐍,𝑥𝜂 (0) =
𝐛2,𝜂 = 𝐍,𝑦𝜂 (0) =
𝐛3,𝜂 = 𝐍,𝑧𝜂 (0) =
𝐛1,𝜁 = 𝐍,𝑥𝜁 (0) =
𝐛2,𝜁 = 𝐍,𝑦𝜁 (0) =
𝐛3,𝜁 = 𝐍,𝑧𝜁 (0) =
[𝐷12𝜸1 + 𝐷13𝛄2],
[𝐷22𝛄1 + 𝐷23𝛄2],
[𝐷32𝛄1 + 𝐷33𝛄2],
[𝐷11𝛄1 + 𝐷13𝛄3],
[𝐷21𝛄1 + 𝐷23𝛄3],
[𝐷31𝛄1 + 𝐷33𝛄3],
[𝐷11𝛄2 + 𝐷12𝛄3],
[𝐷21𝛄2 + 𝐷22𝛄3],
[𝐷31𝛄2 + 𝐷32𝛄3],
𝐛1,𝜉𝜂 = 𝐍,𝑥𝜉𝜂 (0) =
𝐛2,𝜉𝜂 = 𝐍,𝑦𝜉𝜂 (0) =
𝐛3,𝜉𝜂 = 𝐍,𝑧𝜉𝜂 (0) =
𝐛1,𝜂𝜁 = 𝐍,𝑥𝜂𝜁 (0) =
𝐛2,𝜂𝜁 = 𝐍,𝑦𝜂𝜁 (0) =
[𝐷13𝛄4 − (𝐩1
T𝐱𝑖)𝐛𝑖,𝜉 − (𝐫1
T𝐱𝑖)𝐛𝑖,𝜂], 
[𝐷23𝛄4 − (𝐛2
T𝐱𝑖)𝐛𝑖,𝜉 − (𝐫2
T𝐱𝑖)𝐛𝑖,𝜂], 
[𝐷33𝛄4 − (𝐩3
T𝐱𝑖)𝐛𝑖,𝜉 − (𝐫3
T𝐱𝑖)𝐛𝑖,𝜂], 
[𝐷11𝛄4 − (𝐪1
T𝐱𝑖)𝐛𝑖,𝜂 − (𝐩1
T𝐱𝑖)𝐛𝑖,𝜁 ], 
[𝐷21𝛄4 − (𝐪2
T𝐱𝑖)𝐛𝑖,𝜂 − (𝐩2
T𝐱𝑖)𝐛𝑖,𝜁 ], 
(16.18)
(16.19)
(16.20)
(16.21)
(16.22)
(16.23)
(16.24)
(16.25)
(16.26)
(16.27)
(16.28)
(16.29)
(16.30)
(16.31)
(16.32)
(16.33)
(16.34)
LS-DYNA Theory Manual 
Eight-Node Solid Element for Thick Shell Simulations 
𝐛3,𝜂𝜁 = 𝐍,𝑧𝜂𝜁 (0) =
𝐛1,𝜁𝜉 = 𝐍,𝑥𝜁𝜉 (0) =
𝐛2,𝜁𝜉 = 𝐍,𝑦𝜁𝜉 (0) =
𝐛3,𝜁𝜉 = 𝐍,𝑧𝜁𝜉 (0) =
[𝐷31𝛄4 − (𝐪3
T𝐱𝑖)𝐛𝑖,𝜂 − (𝐩3
T𝐱𝑖)𝐛𝑖,𝜁 ], 
[𝐷12𝛄4 − (𝐫1
T𝐱𝑖)𝐛𝑖,𝜁 − (𝐪1
T𝐱𝑖)𝐛𝑖,𝜉 ], 
[𝐷22𝛄4 − (𝐫2
T𝐱𝑖)𝐛𝑖,𝜁 − (𝐪2
T𝐱𝑖)𝐛𝑖,𝜉 ], 
[𝐷32𝛄4 − (𝐫3
T𝐱𝑖)𝐛𝑖,𝜁 − (𝐪3
T𝐱𝑖)𝐛𝑖,𝜉 ], 
where 
and 
𝐩𝑖 = 𝐷𝑖1𝐡1 + 𝐷𝑖3𝐡3,
𝐪𝑖 = 𝐷𝑖1𝐡2 + 𝐷𝑖2𝐡3,
𝐫𝑖 = 𝐷𝑖2𝐡1 + 𝐷𝑖3𝐡2,
𝜸𝛼 = 𝐡𝛼 − (𝐡𝛼
T𝐱𝑖)𝐛𝑖,
T = [1 −1
𝐡1
1 −1
1 −1
1 −1],
T = [1 −1 −1
𝐡2
1 −1
1 −1],
T = [1
𝐡3
1 −1 −1 −1 −1
1],
T = [−1
𝐡4
1 −1
1 −1
1 −1].
(16.35)
(16.36)
(16.37)
(16.38)
(16.39)
(16.40)
(16.41)
(16.42)
(16.43)
(16.44)
(16.45)
(16.46)
In the above equations 𝐡1 is the 𝜉𝜂-hourglass vector, 𝐡2 the 𝜂𝜁 -hourglass vector, 
𝐡3  the 𝜁𝜉 -hourglass  vector and  𝐡4the 𝜉𝜂𝜁 -hourglass  vector.   They  are  the  zero  energy-
deformation modes associated with the one-point-quadrature element which result in a 
non-constant  strain  field  in  the  element  [Flanagan,  1981,  Belytschko,  1984  and  Liu, 
1984].    The  𝛾𝛼  in  equations  (16.21)–(16.38)  are  the  stabilization  vectors.    They  are 
orthogonal to the linear displacement field and provide a consistent stabilization for the 
element. 
The  strain  operators,  𝐁̅̅̅̅̅(𝜉 , 𝜂, 𝜁 ),  can  be  decomposed  into  two  parts,  the 
dilatational part, 𝐁̅̅̅̅̅dil(𝜉 , 𝜂, 𝜁 ), and the deviatoric part, 𝐁̅̅̅̅̅dev(𝜉 , 𝜂, 𝜁 ), both of which can be 
expanded about the element center as in Equation (16.9) 
𝐁̅̅̅̅̅dil(𝛏, 𝛈, 𝛇) = 𝐁̅̅̅̅̅dil(0) + 𝐁̅̅̅̅̅,𝜉
+𝐁̅̅̅̅̅,𝜉𝜂
dil(0)𝛏 + 𝐁̅̅̅̅̅,𝜂
dil (0)𝛇𝛏,
dil (0)𝛈𝛇 + 𝐁̅̅̅̅̅,𝜁𝜉
dil(0)𝛏𝛈 + 𝐁̅̅̅̅̅,𝜂𝜁
dil(0)𝛈 + 𝐁̅̅̅̅̅,𝜁
dil(0)𝛇
(16.47)
Eight-Node Solid Element for Thick Shell Simulations 
LS-DYNA Theory Manual 
𝐁̅̅̅̅̅dev(𝜉 , 𝜂, 𝜁 ) = 𝐁̅̅̅̅̅dev(0) + 𝐁̅̅̅̅̅,𝜉
+𝐁̅̅̅̅̅,𝜉𝜂
dev(0)𝛏𝛈 + 𝐁̅̅̅̅̅,𝜂𝜁
dev(0)𝛈𝛇 + 𝐁̅̅̅̅̅,𝜁𝜉
dev(0)𝜉 + 𝐁̅̅̅̅̅,𝜂
dev(0)𝛇𝛏,
dev(0)𝛈 + 𝐁̅̅̅̅̅,𝜁
dev(0)𝛇
(16.48)
To  avoid  volumetric  locking,  the  dilatational  part  of  the  strain  operators  is 
evaluated only at one quadrature point, the center of the element, i.e., they are constant 
terms 
𝐁̅̅̅̅̅dil(𝝃 , 𝜼, 𝜻) = 𝐁̅̅̅̅̅dil(0).
(16.49)
To  remove  shear  locking,  the  deviatoric  strain  submatrices  can  be  written  in  an 
orthogonal co-rotational coordinate system rotating with the element as 
dev(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑥𝑥
B̅̅̅̅̅𝑥𝑥
+B̅̅̅̅̅𝑥𝑥,𝜉𝜂
dev (0)𝜉𝜂 + B̅̅̅̅̅𝑥𝑥,𝜂𝜁
dev(0) + B̅̅̅̅̅𝑥𝑥,𝜉
dev (0)𝜂𝜁 + B̅̅̅̅̅𝑥𝑥,𝜁𝜉
dev (0)𝜉 + B̅̅̅̅̅𝑥𝑥,𝜂
dev (0)𝜁𝜉 ,
dev (0)𝜂 + B̅̅̅̅̅𝑥𝑥,𝜁
dev (0)𝜁
dev(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑦𝑦
B̅̅̅̅̅𝑦𝑦
+B̅̅̅̅̅𝑦𝑦,𝜉𝜂
dev (0)𝜉𝜂 + B̅̅̅̅̅𝑦𝑦,𝜂𝜁
dev(0) + B̅̅̅̅̅𝑦𝑦,𝜉
dev (0)𝜂𝜁 + B̅̅̅̅̅𝑦𝑦,𝜁𝜉
dev (0)𝜉 + B̅̅̅̅̅𝑦𝑦,𝜂
dev (0)𝜁𝜉 ,
dev (0)𝜂 + B̅̅̅̅̅𝑦𝑦,𝜁
dev (0)𝜁
dev(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑧𝑧
B̅̅̅̅̅𝑧𝑧
+B̅̅̅̅̅𝑧𝑧,𝜉𝜂
dev (0)𝜉𝜂 + B̅̅̅̅̅𝑧𝑧,𝜂𝜁
dev(0) + B̅̅̅̅̅𝑧𝑧,𝜉
dev (0)𝜂𝜁 + B̅̅̅̅̅𝑧𝑧,𝜁𝜉
dev(0)𝜉 + B̅̅̅̅̅𝑧𝑧,𝜂
dev (0)𝜁𝜉 ,
dev(0)𝜂 + B̅̅̅̅̅𝑧𝑧,𝜁
dev(0)𝜁
dev(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑥𝑦
B̅̅̅̅̅𝑥𝑦
dev(0) + B̅̅̅̅̅𝑥𝑦,𝜁
dev (0)𝜁 ,
dev(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑦𝑧
B̅̅̅̅̅𝑦𝑧
dev(0) + B̅̅̅̅̅𝑦𝑧,𝜉
dev (0)𝜉 ,
dev(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑧𝑥
B̅̅̅̅̅𝑧𝑥
dev(0) + B̅̅̅̅̅𝑧𝑥,𝜂
dev (0)𝜂.
(16.50)
(16.51)
(16.52)
(16.53)
(16.54)
(16.55)
Here, only one linear term is left for shear strain components such that the modes 
causing  shear  locking  are  removed.    The  normal  strain  components  keep  all  non-
constant terms given in equation (16.48).   
Summation of equation (16.49) and equations (16.50)–(16.55) yields the following 
strain submatrices which can eliminate the shear and volumetric locking: 
B̅̅̅̅̅𝑥𝑥(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑥𝑥(0) + B̅̅̅̅̅𝑥𝑥,𝜉
+B̅̅̅̅̅𝑥𝑥,𝜉𝜂
dev (0)𝜉𝜂 + B̅̅̅̅̅𝑥𝑥,𝜂𝜁
dev (0)𝜉 + B̅̅̅̅̅𝑥𝑥,𝜂
dev (0)𝜁𝜉 ,
dev (0)𝜂𝜁 + B̅̅̅̅̅𝑥𝑥,𝜁𝜉
dev (0)𝜂 + B̅̅̅̅̅𝑥𝑥,𝜁
dev (0)𝜁
B̅̅̅̅̅𝑦𝑦(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑦𝑦(0) + B̅̅̅̅̅𝑦𝑦,𝜉
+B̅̅̅̅̅𝑦𝑦,𝜉𝜂
dev (0)𝜉𝜂 + B̅̅̅̅̅𝑦𝑦,𝜂𝜁
dev (0)𝜉 + B̅̅̅̅̅𝑦𝑦,𝜂
dev (0)𝜁𝜉 ,
dev (0)𝜂𝜁 + B̅̅̅̅̅𝑦𝑦,𝜁𝜉
dev (0)𝜂 + B̅̅̅̅̅𝑦𝑦,𝜁
dev (0)𝜁
(16.56)
(16.57)
LS-DYNA Theory Manual 
Eight-Node Solid Element for Thick Shell Simulations 
B̅̅̅̅̅𝑧𝑧(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑧𝑧(0) + B̅̅̅̅̅𝑧𝑧,𝜉
+B̅̅̅̅̅𝑧𝑧,𝜉𝜂
dev (0)𝜉𝜂 + B̅̅̅̅̅𝑧𝑧,𝜂𝜁
dev (0)𝜂𝜁 + B̅̅̅̅̅𝑧𝑧,𝜁𝜉
dev (0)𝜁𝜉 ,
dev(0)𝜉 + B̅̅̅̅̅𝑧𝑧,𝜂
dev(0)𝜂 + B̅̅̅̅̅𝑧𝑧,𝜁
dev(0)𝜁
B̅̅̅̅̅𝑥𝑦(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑥𝑦(0) + B̅̅̅̅̅𝑥𝑦,𝜁
dev (0)𝜁 ,
B̅̅̅̅̅𝑦𝑧(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑦𝑧(0) + B̅̅̅̅̅𝑦𝑧,𝜉
dev (0)𝜉 ,
B̅̅̅̅̅𝑧𝑥(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑧𝑥(0) + B̅̅̅̅̅𝑧𝑥,𝜂
dev (0)𝜂.
(16.58)
(16.59)
(16.60)
(16.61)
It  is  noted  that  the  elements  developed  above  cannot  pass  the  patch  test  if  the 
elements are skewed.  To remedy this drawback, the gradient vectors defined in (16.18)–
(16.20) are replaced by the uniform gradient matrices, proposed by Flanagan [1981], 
b̃
⎡
b̃
⎢⎢
b̃
⎣
⎤
⎥⎥
3⎦
=
𝑉𝑒
∫
Ω𝑒
B1(𝜉 , 𝜂, 𝜁 )
⎤
⎡
B2(𝜉 , 𝜂, 𝜁 )
⎥
⎢
B3(𝜉 , 𝜂, 𝜁 )⎦
⎣
𝑑𝑉
. 
Where 𝑉𝑒 is the element volume and the stabilization vector are redefined as 
𝛄̃𝛼 = 𝐡𝛼 − (𝐡𝛼
T𝐱𝑖)𝐛̃
𝑖.
(16.62)
(16.63)
The  element  using  the  strain  submatrices  (16.56)-(16.61)  and  uniform  gradient 
matrices (16.62) with four-point quadrature scheme is called HEXDS element. 
g2
e^
g1
e^
e^
ζ = 0
Figure 16.1.  Definition of co-rotational coordinate system
Eight-Node Solid Element for Thick Shell Simulations 
LS-DYNA Theory Manual 
16.3.2  Co-rotational Coordinate System 
In  elements  for  shell/plate  structure  simulations,  the  elimination  of  the  shear 
locking depends on the proper treatment of the shear strain.  It is necessary to attach a 
local  coordinate  system  to  the  element  so  that  the  strain  tensor  in  this  local  system  is 
relevant for the treatment.  The co-rotational coordinate system determined here is one 
of the most convenient ways to define such a local system. 
A  co-rotational  coordinate  system  is  defined  as  a  Cartesian  coordinate  system 
which  rotates  with  the  element.    Let  {𝑥𝑎, 𝑦𝑎, 𝑧𝑎}  denote  the  current  nodal  spatial 
coordinates  in  the  global  system.    For  each  quadrature  point  with  natural  coordi-
nates(𝜉 , 𝜂, 𝜁 ), we can have two tangent directions on the mid-surface (𝜁 = 0) within the 
element  
𝐠1 =
𝐠2 =
∂𝐱
∂𝜉
∂𝐱
∂𝜂
= [
∂𝑥
∂𝜉
∂𝑦
∂𝜉
∂𝑧
∂𝜉
= [
∂𝑥
∂𝜂
∂𝑦
∂𝜂
∂𝑧
∂𝜂
] = [𝑁𝑎,𝜉 𝑥𝑎 𝑁𝑎,𝜉 𝑦𝑎 𝑁𝑎,𝜉 𝑧𝑎](𝜉,𝜂,0), 
] = [𝑁𝑎,𝜂𝑥𝑎 𝑁𝑎,𝜂𝑦𝑎 𝑁𝑎,𝜂𝑧𝑎](𝜉,𝜂,0). 
(16.64)
(16.65)
The unit vector 𝐞̂1 of the co-rotational coordinate system is defined as the bisector 
of  the  angle  intersected  by  these  two  tangent  vectors  𝐠1  and  𝐠2;  the  unit  vector  𝐞̂3  is 
perpendicular to the mid-surface and the other unit vector is determined by 𝐞̂1 and 𝐞̂3, 
i.e., 
𝐞̂1 = (
𝐠1
∣𝐠1∣
+
𝐠2
∣𝐠2∣
⁄
) (∣
𝐠1
∣𝐠1∣
+
𝐠2
∣𝐠2∣
,
∣)
𝐞̂3 =
𝐠1 × 𝐠2
∣𝐠1 × 𝐠2∣
,
𝐞̂2 = 𝐞̂3 × 𝐞̂1,
which lead to the transformation matrix 
𝐑 =
𝐞̂1
⎤. 
⎡
𝐞̂2
⎥
⎢
𝐞̂3⎦
⎣
(16.66)
(16.67)
(16.68)
(16.69)
16.3.3  Stress and Strain Measures 
Since  the  co-rotational  coordinate  system  rotates  with  the  configuration,  the 
stress  defined  in  this  co-rotational  system  does  not  change  with  the  rotation  or 
translation  of  the  material  body  and  is  thus  objective.    Therefore,  we  use  the  Cauchy 
stress  in  the  co-rotational  coordinate  system,  called  the  co-rotational  Cauchy  stress,  as 
our stress measure.
LS-DYNA Theory Manual 
Eight-Node Solid Element for Thick Shell Simulations 
The  rate  of  deformation  (or  velocity  strain  tensor),  also  defined  in  the  co-
rotational coordinate system, is used as the measure of the strain rate, 
𝛆̇ = 𝐝̂ =
⎡∂𝐯̂def
⎢
∂𝐱̂
⎣
+ (
∂𝐯̂def
∂𝐱̂
)
⎤,
⎥
⎦
(16.70)
where  𝐯̂def  is  the  deformation  part  of  the  velocity  in  the  co-rotational  system  𝐱̂.  If  the 
initial strain 𝛆̂ (𝐗, 0) is given, the strain tensor can be expressed as, 
𝛆̂(X, 𝑡) = 𝛆̂(𝐗, 0) + ∫ 𝐝̂(𝐗, 𝜏)
𝑑𝜏.
(16.71)
The  strain  increment  is  then  given  by  the  mid-point  integration  of  the  velocity 
strain tensor, 
𝑡𝑛+1
𝐝̂𝑑𝜏
=̇
Δ𝛆̂ = ∫
𝑡𝑛
⎡∂Δ𝐮̂def
⎢⎢
∂𝐱̂
⎣
+
⎜⎜⎜⎛∂Δ𝐮̂def
⎟⎟⎟⎞
2 ⎠
∂𝐱̂
⎤
, 
⎥⎥
⎦
𝑛+1
where Δ𝐮̂def is the deformation part of the displacement increment in the co-rotational 
system 𝐱̂𝑛 + 1
 referred to the mid-point configuration. 
𝑛+1
⎝
(16.72)
16.3.4  Co-rotational Stress and Strain Updates 
For  stress  and  strain  updates,  we  assume  that  all variables  at  the previous  time 
step 𝑡𝑛 are known.  Since the stress and strain measures defined in the earlier section are 
objective  in  the  co-rotational  system,  we  only  need  to  calculate  the  strain  increment 
from  the  displacement  field  within  the  time  increment  [𝑡𝑛, 𝑡𝑛 + 1].    The  stress  is  then 
updated by using the radial return algorithm. 
All  the  kinematical  quantities  must  be  computed  from  the  last  time  step 
configuration,  Ω𝑛,  at  𝑡  =   𝑡𝑛  and  the  current  configuration,  Ω𝑛 + 1  at  𝑡  =   𝑡𝑛 + 1  since 
these  are  the  only  available  data.    Denoting  the  spatial  coordinates  of  these  two 
configurations  as  𝐱nand  𝐱n + 1  in  the  fixed  global  Cartesian  coordinate  system  𝑂x,  as 
shown  in  Figure  16.2,  the  coordinates  in  the  corresponding  co-rotational  Cartesian 
coordinate  systems,  𝑂𝐱̂𝑛  and  𝑂𝐱̂𝑛 + 1,  can  be  obtained  by  the  following  transformation 
rules: 
𝐱̂𝑛 = 𝐑𝑛𝐱𝑛,
𝐱̂𝑛+1 = 𝐑𝑛+1𝐱𝑛+1,
(16.73)
(16.74)
where 𝐑𝑛 and 𝐑𝑛 + 1 are the orthogonal transformation matrices which rotate the global 
coordinate system to the corresponding co-rotational coordinate systems, respectively.
Eight-Node Solid Element for Thick Shell Simulations 
LS-DYNA Theory Manual 
n+1
n+1/2
^
n+1
^
n+1/2
^
Xn
Figure 16.2.  Configurations at times 𝑡𝑛, 𝑡𝑛 + 1
, and 𝑡𝑛+1, 
Since  the  strain  increment  is  referred  to  the  configuration  at  𝑡  =   𝑡𝑛 + 1
assuming the velocities within the time increment [𝑡𝑛, 𝑡𝑛 + 1] are constant, we have 
,  by 
=
𝑛+1
(𝐱𝑛 + 𝐱𝑛+1),
(16.75)
and  the  transformation  to  the  co-rotational  system  associated  with  this  mid-point 
configuration, Ω𝑛 + 1
, is given by 
𝐱̂
𝑛+1
= 𝐑
𝑛+1
.
𝑛+1
(16.76)
Similar  to  polar  decomposition,  an  incremental  deformation  can  be  separated 
into  the  summation  of  a  pure  deformation  and  a  pure  rotation  [Belytschko,  1973].  
Letting  Δ𝐮  indicate  the  displacement  increment  within  the  time  increment  [𝑡𝑛, 𝑡𝑛 + 1
we write 
], 
Δ𝐮 = Δ𝐮def + Δ𝐮rot,
(16.77)
where Δ𝐮def and Δ𝐮rot are, respectively, the deformation part and the pure rotation part 
of  the  displacement  increment  in  the  global  coordinate  system.    The  deformation  part 
also includes the translation displacements which cause no strains.
LS-DYNA Theory Manual 
Eight-Node Solid Element for Thick Shell Simulations 
In order to obtain the deformation part of the displacement increment referred to 
,  we  need  to  find  the  rigid  rotation  from  Ω𝑛  to  Ω𝑛 + 1 
,  is  held  still.    Defining  two  virtual 
the  configuration  at  𝑡 = 𝑡𝑛 + 1
provided  that  the  mid-point  configuration,  Ω𝑛 + 1
configurations,  Ω′𝑛  and  Ω′𝑛 + 1,  by  rotating  the  element  bodies  Ω𝑛  and  Ω𝑛 + 1  into  the 
  (Fig.    13.3)  and  denoting  and  𝐱′̂
co-rotational  system  𝑂x̂𝑛 + 1
𝑛 + 1  as  the  coordinates  of 
Ω′𝑛 and Ω′𝑛 + 1 in the co-rotational system 𝑂𝐱̂𝑛 + 1
, we have 
𝐱′̂
𝑛 =   𝐱̂𝑛,
𝐱′̂
𝑛 + 1 = 𝐱̂𝑛 + 1.
(16.78)
We can see that from Ω𝑛 to Ω′𝑛 and from Ω′𝑛 + 1 to Ω𝑛 + 1, the body experiences 
two rigid rotations and the rotation displacements are given by 
Δ𝐮1
rot = 𝐱′𝑛 − 𝐱𝑛 = 𝐑
𝑛 − 𝐱𝑛 = 𝐑
T 𝐱′̂
𝑛+1
T 𝐱̂𝑛 − 𝐱𝑛,
𝑛+1
Δ𝐮2
rot = 𝐱𝑛+1 − 𝐱′𝑛+1 = 𝐱𝑛+1 − 𝐑
𝑛+1 = 𝐱𝑛+1 − 𝐑
T 𝐱′̂
𝑛+1
T 𝐱̂𝑛+1. 
𝑛+1
Thus the total rotation displacement increment can be expressed as 
T (𝐱̂𝑛+1 − 𝐱̂𝑛)
𝑛+1
rot = 𝐱𝑛+1 − 𝐱𝑛 − 𝐑
Δ𝐮rot = Δ𝐮1
rot + Δ𝐮2
= Δ𝐮 − 𝐑
T (𝐱̂𝑛+1 − 𝐱̂𝑛).
𝑛+1
(16.79)
(16.80)
(16.81)
Then  the  deformation  part  of  the  displacement  increment  referred  to  the 
configuration Ω𝑛 + 1
 is 
Δ𝐮def = Δ𝐮 − Δ𝐮rot = 𝐑
T (𝐱̂𝑛+1 − 𝐱̂𝑛).
𝑛+1
(16.82)
Therefore,  the  deformation  displacement 
increment 
in  the  co-rotational 
coordinate system 𝑂x̂𝑛 + 1
 is obtained as  
Δ𝐮̂def = 𝐑
𝑛+1
Δ𝐮def = 𝐱̂𝑛+1 − 𝐱̂𝑛.
(16.83)
Once  the  strain  increment  is  obtained  by  equation  (16.72),  the  stress  increment, 
also  referred  to  the  mid-point  Configuration,  can  be  calculated  with  the  radial  return 
algorithm.  The total strain and stress can then be updated as 
𝛆̂𝑛+1 = 𝛆̂𝑛 + Δ𝛆̂,
𝛔̂𝑛+1 = 𝛔̂𝑛 + Δ𝛔̂.
(16.84)
(16.85)
Eight-Node Solid Element for Thick Shell Simulations 
LS-DYNA Theory Manual 
n+1
Δu
Pn+1
rot
Δu2
,
n+1
n+1/2
Δudef
n+1
^
Ω,
n+1
^
n+1/2
,
Ω,
rot
Δu1
Pn
^
Figure 16.3.  Separation of the displacement increment 
Note that the resultant stress and strain tensors are both referred to the current 
configuration and defined in the current co-rotational coordinate system.  By using the 
tensor transformation rule we can have the strain and stress components in the global 
coordinate system.   
  Tangent Stiffness Matrix and Nodal Force Vectors 
From  the  Hu-Washizu  variational  principle,  at  both  𝑣th  and  (𝑣 + 1)th  iteration, 
we have 
∫ 𝛿𝜀̂𝑖𝑗
Ω̂𝑣
𝑣 𝜎̂𝑖𝑗
𝑣 ,
𝑑𝑉 = 𝛿𝜋̂ext
∫
Ω̂𝑣+1
𝛿𝜀̂𝑖𝑗
𝑣+1𝜎̂𝑖𝑗
𝑣+1
𝑑𝑉 = 𝛿𝜋̂ext
𝑣+1,
(16.86)
(16.87)
where 𝛿𝜋̂ext  is  the  virtual work  done  by  the external  forces.   Note  that  both  equations 
are  written  in  the  co-rotational  coordinate  system  defined  in  the  𝑣th  iterative 
configuration  given  by  x𝑛+1
.    The  variables  in  this  section  are  within  the  time  step 
[𝑡𝑛, 𝑡𝑛+1
] and superscripts indicate the number of iterations. 
Assuming  that  all  external  forces  are  deformation-independent,  linearization  of 
Equation (16.87) gives [Liu, 1992]
LS-DYNA Theory Manual 
Eight-Node Solid Element for Thick Shell Simulations 
∫ 𝛿𝑢̂𝑖,𝑗
Ω̂𝑣
𝑣 𝐶̂
𝑣 Δ𝑢̂𝑘,𝑙𝑑𝑉 +
𝑖𝑗𝑘𝑙
∫ 𝛿𝑢̂𝑖,𝑗
Ω̂𝑣
𝑣 𝑇̂
𝑣 Δ𝑢̂𝑘,𝑙𝑑𝑉 = 𝛿𝜋̂ext
𝑖𝑗𝑘𝑙
𝑣+1 −
𝑣 , 
𝛿𝜋̂ext
where the Green-Naghdi rate of Cauchy stress tensor is used, i.e., 
𝑇̂
𝑣.
𝑣 = 𝛿𝑖𝑘𝜎̂𝑗𝑙
𝑖𝑗𝑘𝑙
(16.88)
(16.89)
The first term on the left hand side of (16.88) denotes the material response since 
it  is  due  to  pure  deformation  or  stretching;  the  second  term  is  an  initial  stress  part 
resulting from finite deformation effect.   
Taking account of the residual of the previous iteration, Equation (16.87) can be 
approximated as  
∫ 𝛿𝑢̂𝑖,𝑗
Ω̂𝑣
𝑣 (𝐶̂
𝑣 + 𝑇̂
𝑖𝑗𝑘𝑙
𝑣 )Δ𝑢̂𝑘,𝑙
𝑖𝑗𝑘𝑙
𝑑𝑉 = 𝛿𝜋̂ext
𝑣+1 − ∫ 𝛿𝜀̂𝑖𝑗
𝑣 𝜎̂𝑖𝑗
𝑣𝑑𝑉
Ω̂𝑣
.
(16.90)
If the strain and stress vectors are defined as  
𝛆T = [𝜀𝑥
𝜀𝑦
𝜀𝑧
2𝜀𝑥𝑦
2𝜀𝑦𝑧
2𝜀𝑧𝑥
2𝜔𝑥𝑦
2𝜔𝑦𝑧
2𝜔𝑧𝑥], 
𝛔T = [𝜎𝑥 𝜎𝑦 𝜎𝑧 𝜎𝑥𝑦 𝜎𝑦𝑧 𝜎𝑧𝑥],
(16.91)
(16.92)
We can rewrite equation (16.90) as  
∫ 𝛿𝜀̂𝑖
Ω̂𝑣
𝑣(𝐶̂𝑖𝑗
𝑣 + 𝑇̂𝑖𝑗
𝑣)𝛿𝜀̂𝑗
𝑑𝑉 = 𝛿𝜋̂ext
𝑣+1 − ∫ 𝛿𝜀̂𝑖
𝑣𝜎̂𝑗
𝑣𝑑𝑉
Ω̂𝑣
,
(16.93)
𝑣 is the consistent tangent modulus tensor corresponding to pure deformation 
𝑣 is the geometric stiffness matrix 
where 𝐶̂𝑖𝑗
 but expanded to a 9 by 9 matrix; 𝑇̂𝑖𝑗
which is given as follows [Liu 1992]:
Eight-Node Solid Element for Thick Shell Simulations 
LS-DYNA Theory Manual 
𝜎2
𝜎3
𝜎4
𝜎4
𝜎1   +   𝜎2
𝜎5
𝜎5
𝜎6
𝜎2   +   𝜎3
symm.
𝜎6
𝜎6
𝜎5
𝜎4
𝜎1   +   𝜎3
𝜎4
𝜎4
−
𝜎2   −   𝜎1
𝜎6
−
𝜎5
𝜎1   +   𝜎2
T  =  
⎡𝜎1
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
𝜎5
𝜎5
−
𝜎6
𝜎3   −   𝜎2
𝜎4
𝜎6
𝜎2   +   𝜎3
−
−
−
𝜎6
𝜎6
𝜎5
−
𝜎4
𝜎1   −   𝜎3
𝜎5
𝜎4
𝜎3   +   𝜎1
−
−
(16.94)
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
.
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎦
By interpolation 
Δ𝐮 = 𝐍Δ𝐝,
𝛿𝐮 = 𝐍𝛿𝐝;
(16.95)
(16.96)
where  𝐍  and  𝐁̅̅̅̅̅  are,  respectively,  the  shape  functions  and  strain  operators  defined  in 
Section 2.  This leads to a set of equations  
Δ𝛆 = 𝐁̅̅̅̅̅Δ𝐝,
𝛿𝛆 = 𝐁̅̅̅̅̅𝛿𝐝,
𝐊̂𝑣Δ𝐝̂ = 𝐫 ̂𝑣+1 = 𝐟 ̂
𝑣+1 − 𝐟 ̂
ext
𝑣 ,
int
(16.97)
where the tangent stiffness matrix, 𝐊̂𝑣, and the internal nodal force vector, 𝐟 ̂
𝑣 , are  
int
𝐊̂𝑣 = ∫ 𝐁̅̅̅̅̅̂T(𝐂̂𝑣 + 𝐓̂𝑣)𝐁̅̅̅̅̅̂dV
Ω̂𝑣
,
𝑣 = ∫ 𝐁̅̅̅̅̅̂T𝛔̂𝑣dV
𝐟 ̂
int
Ω̂𝑣
.
(16.98)
(16.99)
The tangent stiffness and nodal force are transformed into the global coordinate 
system tensorially as  
𝐊𝑣 = 𝐑𝑣T𝐊̂𝑣𝐑𝑣,
𝑣 ,
𝐫𝑣+1 = 𝐑𝑣T𝐫 ̂int
(16.100)
(16.101)
where  𝐑𝑣  is  the  transformation  matrix  of  the  co-rotational  system  defined  by  𝐱𝑛+1
Finally, we get a set of linear algebraic equations 
.
LS-DYNA Theory Manual 
Eight-Node Solid Element for Thick Shell Simulations 
𝐊𝑣Δ𝐝𝑣+1 = 𝐫𝑣+1.
(16.102)
16.4  Numerical Examples 
To investigate the performance of the element introduced in this paper, a variety 
of  problems  including  linear  elastic  and  nonlinear  elastic-plastic/large  deformation 
problems are studied.  Since the element is developed to avoid locking, the applicability 
to  problems  of  thin  structures  is  studied  by  solving  the  standard  test  problems 
including  pinched  cylinder  and  Scordelis-Lo  roof,  which  are  proposed  by  MacNeal, 
1985 and Belytschko, 1984b.  Also a sheet metal forming problem is solved to test and 
demonstrate the effectiveness and efficiency of this element.   
16.4.1  Timoshenko Cantilever Beam 
The  first  problem  is  a  linear,  elastic  cantilever  beam  with  a  load  at  its  end  as 
shown in Fig. 16.4, where 𝑀 and 𝑃 at the left end of the cantilever are reactions at the 
support.  The analytical solution from Timoshenko, 1970 is  
𝑢𝑥(𝑥, 𝑦) =
−𝑃𝑦
6𝐸̅̅̅̅𝐼
[(6𝐿 − 3𝑥)𝑥 + (2 + 𝑣̅) (𝑦2 −
𝐷2)],
(16.103)
𝑢𝑦(𝑥, 𝑦) =
6𝐸̅̅̅̅𝐼
[3𝑣̅𝑦2(𝐿 − 𝑥) +
(4 + 5𝑣̅)𝐷2𝑥 + (3𝐿 − 𝑥)𝑥2], 
(16.104)
where 
𝐼 =
12
𝐷3,
𝐸̅̅̅̅   =   {
𝐸,
𝐸/(1  −   𝑣2) ,
 𝑣̅   =  
{⎧
⎩{⎨
1 − 𝑣
for plane stress
for plane strain
(16.105)
(16.106)
The displacements at the support end, 𝑥 = 0, −  1
2 𝐷 are nonzero except 
at the top, bottom and midline (as shown in Fig.  13.5).  Reaction forces are applied at 
the  support  based  on  the  stresses  corresponding  to  the  displacement  field  at  𝑥 = 0, 
which are 
2 𝐷 ≤ 𝑦 ≤   1
𝜎𝑥𝑥 = −
𝑃𝑦
(𝐿 − 𝑥),
𝜎𝑦𝑦 = 0,
𝜎𝑥𝑦 =
2𝐼
(
𝐷2 − 𝑦2). 
(16.107)
The  distribution  of  the  applied  load  to the  nodes  at 𝑥 = 𝐿  is  also  obtained  from 
the closed-form stress fields.
Eight-Node Solid Element for Thick Shell Simulations 
LS-DYNA Theory Manual 
Figure 16.4.  Timoshenko cantilever beam. 
D/2
D/2
(a) Regular mesh
L/4
(b) Skewed mesh
p/2
Pt. A
p/2
Pt. A
Figure 16.5.  Top half of anti-symmetric beam mesh 
The  parameters  for  the  cantilever  beam  are:  𝐿 = 1.0, 𝐷 = 0.02, 𝑃 = 2.0, 𝐸 = 1 ×
107; and two values of Poisson’s ratio: (1)𝑣 = 0.25, (2)𝑣 = 0.4999.   
Since  the  problem  is  anti-symmetric,  only  the  top  half  of  the  beam  is  modeled.  
Plane strain conditions are assumed in the z-direction and only one layer of elements is 
used in this direction.  Both regular mesh and skewed mesh are tested for this problem.   
Normalized  vertical  displacements  at  point  A  for  each  case  are  given  in  Table 
13.1.    Tables 13.1a  and  13.1b  show  the  normalized  displacement  at  point  A  for  the
LS-DYNA Theory Manual 
Eight-Node Solid Element for Thick Shell Simulations 
regular mesh.  There is no shear or volumetric locking for this element.  For the skewed 
mesh,  with  the  skewed  angle  increased,  we  need  more  elements  to  get  more  accurate 
solution (Table 13.1c).   
(a) 𝑣 = 0.25, regular mesh 
       Analytical solution 𝑤A = 9.3777 × 10−2 
Mesh 
4 × 1 × 1
8 × 1 × 1 
8 × 2 × 1 
HEXDS 
1.132 
1.142 
1.029 
(b) 𝑣 = 0.4999, regular mesh 
       Analytical solution 𝑤A = 7.5044 × 10−2 
Mesh 
4 × 1 × 1
8 × 1 × 1 
8 × 2 × 1 
HEXDS 
1.182 
1.197 
1.039 
(c) 𝑣 = 0.25, skewed mesh 
1° 
5° 
10° 
4 × 1 ×1 
8 × 1 ×1 
1.078 
0.580 
0.317 
1.136 
0.996 
0.737 
16 × 1 ×1 
1.142 
1.090 
.955 
Table 13.1.  Normalized displacement at point A of cantilever beam.
Eight-Node Solid Element for Thick Shell Simulations 
LS-DYNA Theory Manual 
16.4.2  Pinched Cylinder 
Figure  16.6  shows  a  pinched  cylinder  subjected  to  a  pair  of  concentrated  loads.  
Two  cases  are  studied  in  this  example.    In  the  first  case,  both  ends  of  the  cylinder  are 
assumed to be free.  In the second case, both ends of the cylinder are covered with rigid 
diaphragms so that only the displacement in the axial direction is allowed at the ends.  
The parameters for the first case  
(without diaphragms) are 
𝐸 = 1.05 × 106, 𝑣 = 0.3125, 𝐿 = 10.35, 𝑅 = 1.0, 𝑡 = 0.094, 𝑃 = 100.0; 
(16.108)
while for the second case (with diaphragms), the parameters are set to be 
𝐸 = 3 × 106, 𝑣 = 0.3, 𝐿 = 600.0, 𝑅 = 300.0, 𝑡 = 3.0, 𝑃 = 1.0. 
(16.109)
Due  to  symmetry  only  one  octant  of  the  cylinder  is  modeled.    The  computed 
displacements at the loading point are compared to the analytic solutions in Table 13.2. 
HEXDS  element  works  well  in  both  cases,  indicating  that  this  element  can  avoid  not 
only shear locking but also membrane locking; this is not unexpected since membrane 
locking occurs primarily in curved elements [Stolarski, 1983].   
16.4.3  Scordelis-Lo Roof 
Scordelis-Lo roof subjected to its own weight is shown in Figure 16.7.  Both ends 
of  the  roof  are  assumed  to  be  covered  with  rigid  diaphragms.    The  parameters  are 
selected  to  be:  𝐸 = 4.32 × 108, 𝑣  =  0.0, 𝐿  =  50.0, 𝑅 = 25.0, 𝑡  =  0.25, 𝜃  =  40∘,  and 
the gravity is 360.0 per volume. 
free or with diaphragm
m etric
sy m
symmetric
m etric
sy m
Figure 16.6.  Pinched cylinder and the element model
LS-DYNA Theory Manual 
Eight-Node Solid Element for Thick Shell Simulations 
2L
Figure 16.7.  Scordelis-Lo roof under self-weight 
 (a) First case without diaphragms 
        Analytical solution 𝑤max = 0.1137 
Mesh 
10 × 10 × 2 
16 × 16 × 4 
20 × 20 × 4 
HEXDS 
1.106 
1.054 
1.067 
(b) Second case with diaphragms 
        Analytical solution wmax = 1.8248 × 10−5 
Mesh 
10 × 10 × 2 
16 × 16 × 4 
20 × 20 × 4 
HEXDS 
0.801 
0.945 
.978 
Table 13.2.  Normalized displacement at loading point of pinched cylinder 
Due  to  symmetry  only  one  quarter  of  the  roof  is  modeled.    The  computed 
displacement at the midpoint of the edge is compared to the analytic solution in Table 
13.3.  In this example the HEXDS element can get good result with 100 × 2 elements.
Eight-Node Solid Element for Thick Shell Simulations 
LS-DYNA Theory Manual 
R0=50.8mm
t=2mm
tight die
r=2mm
Rd=54mm
R=54mm
Figure 16.8.  Circular sheet stretched with a tight die 
Analytical solution 𝑤max = 0.3024 
Mesh 
8 × 8 × 1 
16 × 16 × 1 
32 × 32 × 1 
10 × 10 × 2 
HEXDS 
1.157 
1.137 
1.132 
1.045 
16.4.4  Circular Sheet Stretched with a Tight Die 
A  circular  sheet  is  stretched  under  a  hemisphere  punch  and  a  tight  die  with  a 
small  corner  radius  (Fig.  16.8).    The  material  is  elastoplastic  with  nonlinear  hardening 
rule.  The elastic material constants are: 𝐸 = 206 GPa and 𝑣 = 0.3.  In the plastic range, 
the uniaxial stress-strain curve is given by  
𝜎 = 𝐾𝜀𝑛,
(16.110)
where  𝐾 = 509.8MPa, 𝑛 = 0.21,  𝜎  is  Cauchy  stress  and  𝜀  is  natural  strain  (logarithmic 
strain).    The  initial  yield  stress  is  obtained  to  be  𝜎0 = 103.405Mpa  and  the  tangent 
modulus at the initial yield point is 𝐸t = 0.4326 × 105MPa. 
Because  of  the  small  corner  radius  of  the  die,  the  same  difficulties  as  in  the 
problem  of  sheet  stretch  under  the  rigid  cylinders  lead  the  shell  elements  to  failure  in 
this problem.  Three-dimensional solid elements are needed and fine meshes should be 
put in the areas near the center and the edge of the sheet.   
One  quarter  of  the  sheet  is  modeled  with  1400  ×  2  HEXDS  elements  due  to  the 
double symmetries.  The mesh is shown in Fig. 16.9.  Two layers of elements are used in 
the  thickness.    Around  the  center  and  near the  circular  edge  of the  sheet,  fine  mesh  is 
used.  The nodes on the edge are fixed in x- and y-directions and the bottom nodes on 
the edge are prescribed in three directions.  No friction is considered in this simulation.
LS-DYNA Theory Manual 
Eight-Node Solid Element for Thick Shell Simulations 
Figure 16.9.  Mesh for circular sheet stretching 
For  comparison,  the  axisymmetric  four-node  element  with  reduced  integration 
(CAX4R) is also used and the mesh for this element is the same as shown in the top of 
Figure 13.9. 
The  results  presented  here  are  after  the  punch  has  traveled  down  50  mm.    The 
profile  of  the  circular  sheet  is  shown  in  Figure  16.10  where  we  can  see  that  the  sheet 
  Figure 16.10.  Deformed shape of a circular sheet with punch travel 50 mm 
under the punch experiences most of the stretching and the thickness of the sheet above
Eight-Node Solid Element for Thick Shell Simulations 
LS-DYNA Theory Manual 
Figure 16.11.  Reaction force vs.  punch travel for the circular sheet 
the  die  changes  a  lot.    The  deformation  between  the  punch  and  the  die  is  small.  
However,  the  sheet  thickness  obtained  by  the  CAX4R  element  is  less  than  that  by  the 
HEXDS element and there is slight difference above the die.  These observations can be 
verified by the strain distributions in the sheet along the radial direction (Figure 13.12).  
The direction of the radial strain is the tangent of the mid-surface of the element in the 
rz plane and the thickness strain is in the direction perpendicular to the mid-surface of 
the element.  The unit vector of the circumferential strain is defined as the cross-product 
of the directional cosine vectors of the radial strain and the thickness strain.  We can see 
that  the  CAX4R  element  yields  larger  strain  components  in  the  area  under  the  punch 
than the HEXDS element.  The main difference of the strain distributions in the region 
above  the  die  is  that  the  CAX4R  element  gives  zero  circumferential  strain  in  this  area 
but the HEXDS element yields non-zero strain.  The value of the reaction force shown in 
the  Figure  13.11  is  only  one  quarter  of  the  total  punch  reaction  force  since  only  one 
quarter  of  the  sheet  is  modeled.    From  this  figure  we  can  see  that  the  sheet  begins 
softening after the punch travels down about 45 mm, indicating that the sheet may have 
necking though this cannot be seen clearly from Figure 16.10.
LS-DYNA Theory Manual 
Eight-Node Solid Element for Thick Shell Simulations 
(a) Radial strain distribution 
(b) Circumferential strain distribution 
(c) Thickness strain distribution 
Figure 13.12.  Strain distributions in circular sheet with punch travel 50 mm
Eight-Node Solid Element for Thick Shell Simulations 
LS-DYNA Theory Manual 
16.5  Conclusions 
A new eight-node hexahedral element is implemented for the large deformation 
elastic-plastic analysis.  Formulated in the co-rotational coordinate system, this element 
is shown to be effective and efficient and can achieve fast convergence in solving a wide 
variety of nonlinear problems.   
By  using  a  co-rotational  system  which  rotates  with  the  element,  the  locking 
phenomena  can  be  suppressed  by  omitting  certain  terms  in  the  generalized  strain 
operators.  In addition, the integration of the constitutive equation in the co-rotational 
system  takes  the  same  simple  form  as  small  deformation  theory  since  the  stress  and 
strain tensors defined in this co-rotational system are objective. 
Radial  return  algorithm  is  used  to  integrate  the  rate-independent  elastoplastic 
constitutive  equation.    The  tangent  stiffness  matrix  consistently  derived  from  this 
integration  scheme  is  crucial  to  preserve  the  second  order  convergence  rate  of  the 
Newton’s iteration method for the nonlinear static analyses.   
Test  problems  studied  in  this  paper  demonstrate  that  the  element  is  suitable  to 
continuum and structural numerical simulations.  In metal sheet forming analysis, this 
element  has  advantages  over  shell  elements  for  certain  problems  where  through  the 
thickness deformation and strains are significant.
LS-DYNA Theory Manual 
Truss Element 
17    
Truss Element 
One  of  the  simplest  elements  is  the  pin-jointed  truss  element  shown  in 
Figure 17.1.  This element has three degrees of freedom at each node and carries an axial 
force.  The displacements and velocities measured in the local system are interpolated 
along the axis according to 
𝑢 = 𝑢1 +
(𝑢2 − 𝑢1),
where at 𝑥 = 0, 𝑢 = 𝑢1 and at 𝑥 = 𝐿, 𝑢 = 𝑢2.  Incremental strains are found from 
(𝑢̇2 − 𝑢̇1),
𝑢̇ = 𝑢̇1 +
and are computed in LS-DYNA using 
Δ𝜀 =
(𝑢̇2 − 𝑢̇1)
Δ𝑡
Δ𝜀𝑛+1
2⁄ =
2 (𝑢̇2
𝑛+1
2⁄
𝑛+1
2⁄
− 𝑢̇1
𝐿𝑛 + 𝐿𝑛+1
)
Δ𝑡𝑛+1
2⁄
(17.1)
(17.2)
(17.3)
(17.4)
The  normal  force  𝑁  is  then  incrementally  updated  using  a  tangent  modulus  𝐸𝑡 
according to 
𝑁𝑛+1 = N𝑛𝐴𝐸𝑡 + Δ𝜀𝑛+1/2
(17.5)
Truss Element 
N1
LS-DYNA Theory Manual 
u1
N2
u2
Figure 17.1.  Truss element. 
Two  constitutive  models  are  implemented  for  the  truss  element:  elastic  and 
elastic-plastic with kinematic hardening.
LS-DYNA Theory Manual 
Membrane Element 
18    
Membrane Element 
The  Belytschko-Lin-Tsay  shell  element  {Belytschko  and  Tsay  [1981],  Belytschko 
et al., [1984a]} is the basis for this very efficient membrane element.  In this section we 
briefly  outline  the  theory  employed  which,  like  the  shell  on  which  it  is  based,  uses  a 
combined co-rotational and velocity-strain formulation.  The efficiency of the element is 
obtained  from  the  mathematical  simplifications  that  result  from  these  two  kinematical 
assumptions.    The  co-rotational  portion  of  the  formulation  avoids  the  complexities  of 
nonlinear mechanics by embedding a coordinate system in the element.  The choice of 
velocity  strain  or  rate  of  deformation  in  the  formulation  facilitates  the  constitutive 
evaluation, since the conjugate stress is the more familiar Cauchy stress.   
In membrane elements the rotational degrees of freedom at the nodal points may 
be  constrained,  so  that  only  the  translational  degrees-of-freedom  contribute  to  the 
straining  of  the  membrane.    A  triangular  membrane  element  may  be  obtained  by 
collapsing adjacent nodes of the quadrilateral. 
18.1  Co-rotational Coordinates 
The  mid-surface  of  the  quadrilateral  membrane  element  is  defined  by  the 
location of the element’s four corner nodes.  An embedded element coordinate system 
(Figure  7.1)  that  deforms  with  the  element  is  defined  in  terms  of  these  nodal 
coordinates.  The co-rotational coordinate system follows the development in Section 7, 
Equations (7.1)—(7.3).
Membrane Element 
LS-DYNA Theory Manual 
18.2  Velocity-Strain Displacement Relations 
The  co-rotational  components  of  the  velocity  strain  (rate  of  deformation)  are 
given by: 
𝑑 ̂
𝑖𝑗 =
(
∂𝜐̂𝑖
∂𝑥̂𝑗
+
∂𝜐̂𝑗
∂𝑥̂𝑖
),
(18.1)
The  above  velocity-strain  relations  are  evaluated  only  at  the  center  of  the  shell.  
Standard bilinear nodal interpolation is used to define the mid-surface velocity, angular 
  These 
velocity,  and  the  element’s  coordinates  (isoparametric  representation). 
interpolation relations are given by 
𝑣𝑚 = 𝑁𝐼(𝜉 , 𝜂)𝑣𝐼,
𝑥𝑚 = 𝑁𝐼(𝜉 , 𝜂)𝑥𝐼,
(18.2)
(18.3)
where the subscript 𝐼 is summed over all the element’s nodes and the nodal velocities 
are  obtained  by  differentiating  the  nodal coordinates  with  respect  to  time,  i.e., 𝜐𝐼 = ẋ𝐼.  
The bilinear shape functions are defined in Equations (7.10). 
The  velocity  strains  at  the  center  of  the  element,  i.e.,  at  𝜉 = 0,  and  𝜂 = 0,  are 
obtained as in Section 7 giving: 
where 
𝑑 ̂
𝑥 = 𝐵1𝐼𝜐̂𝑥𝐼,
𝑑 ̂
𝑦 = 𝐵2𝐼𝜐̂𝑦𝐼,
2𝑑 ̂
𝑥𝑦 = 𝐵2𝐼𝑣̂𝑥𝐼 + 𝐵1𝐼𝑣̂𝑦𝐼,
𝐵1𝐼 =
𝐵2𝐼 =
∂𝑁𝐼
∂𝑥̂
,
∂𝑁𝐼
∂𝑦̂
.
(18.4)
(18.5)
(18.6)
(18.7)
(18.8)
18.3  Stress Resultants and Nodal Forces 
After  suitable  constitutive  evaluations  using  the  above  velocity  strains,  the 
resulting  stresses  are  multiplied  by  the  thickness  of  the  membrane,  h,  to  obtain  local 
resultant forces.  Therefore,  
18-2 (Membrane Element) 
𝑓 ̂
𝑅 = ℎ𝜎̂𝛼𝛽,
𝛼𝛽
LS-DYNA Theory Manual 
Membrane Element 
where the superscript R indicates a resultant force and the Greek subscripts emphasize 
the limited range of the indices for plane stress plasticity. 
The above element centered force resultants are related to the local nodal forces 
by 
𝑅 + 𝐵2𝐼𝑓 ̂
𝑥𝐼 = 𝐴(𝐵1𝐼𝑓 ̂
𝑓 ̂
𝑅 ),
𝑥𝑦
𝑥𝑥
𝑅 + 𝐵1𝐼𝑓 ̂
𝑦𝐼 = 𝐴(𝐵2𝐼𝑓 ̂
𝑓 ̂
𝑅 ),
𝑥𝑦
𝑦𝑦
(18.10)
(18.11)
where 𝐴 is the area of the element. 
The  above  local  nodal  forces  are  then  transformed  to  the  global  coordinate 
system using the transformation relations given in Equation (7.5a). 
18.4  Membrane Hourglass Control 
Hourglass  deformations  need  to  be  resisted  for  the  membrane  element.    The 
hourglass control for this element is discussed in Section 7.4.
LS-DYNA Theory Manual 
Discrete Elements and Masses 
19    
Discrete Elements and Masses 
The discrete elements and masses in LS-DYNA provide a capability for modeling 
simple spring-mass systems as well as the response of more complicated mechanisms.  
Occasionally,  the  response  of  complicated  mechanisms  or  materials  needs  to  be 
included  in  LS-DYNA  models,  e.g.,  energy  absorbers  used  in  passenger  vehicle 
bumpers.  These mechanisms are often experimentally characterized in terms of force-
displacement  curves.    LS-DYNA  provides  a  selection  of  discrete  elements  that  can  be 
used individually or in combination to model complex force-displacement relations. 
The  discrete  elements  are  assumed  to  be  massless.    However,  to  solve  the 
equations of motion at unconstrained discrete element nodes or nodes joining multiple 
discrete elements, nodal masses must be specified at these nodes.  LS-DYNA provides a 
direct method for specifying these nodal masses in the model input. 
All  of  the  discrete  elements  are  two-node  elements,  i.e.,  three-dimensional 
springs  or  trusses.    A  discrete  element  may  be  attached  to  any  of  the  other  LS-DYNA 
continuum,  structural,  or  rigid  body  element.    The  force  update  for  the  discrete 
elements may be written as 
𝐟 ̂𝑖+1 = 𝐟 ̂𝑖 + Δ𝐟 ̂,
(19.1)
where  the  superscript  𝑖 + 1  indicates  the  time  increment  and  the  superposed  caret  (⋅ ̂) 
indicates the force in the local element coordinates, i.e., along the axis of the element.  In 
the default case, i.e., no orientation vector is used; the global components of the discrete 
element force are obtained by using the element’s direction cosines: 
{⎧𝐹𝑥
}⎫
𝐹𝑦
𝐹𝑧⎭}⎬
⎩{⎨
   =
𝑓 ̂
{⎧Δ𝑙𝑥
}⎫
Δ𝑙𝑦
}⎬
{⎨
Δ𝑙𝑧⎭
⎩
{⎧𝑛𝑥
}⎫
= 𝑓 ̂
𝑛𝑦
𝑛𝑧⎭}⎬
⎩{⎨
= 𝑓 ̂𝐧
~
, 
(19.2)
where
Discrete Elements and Masses 
LS-DYNA Theory Manual 
Δ𝐥 =
{⎧Δ𝑙𝑥
}⎫
Δ𝑙𝑦
}⎬
{⎨
Δ𝑙𝑧⎭
⎩
=  
{⎧𝑥2 − 𝑥1
}⎫
𝑦2 − 𝑦1
𝑧2 − 𝑧1 ⎭}⎬
⎩{⎨
. 
𝑙 is the length  
𝑙 = √Δ𝑙𝑥
2 + Δ𝑙𝑦
2,
2 + Δ𝑙𝑧
(19.3)
(19.4)
and (𝑥𝑖, 𝑦𝑖, 𝑧𝑖) are the global coordinates of the nodes of the spring element.  The forces 
in Equation (19.2) are added to the first node and subtracted from the second node. 
For  a  node  tied  to  ground  we  use  the  same  approach  but  for  the  (𝑥2, 𝑦2, 𝑧2) 
coordinates in Equation (19.2) the initial coordinates of node 1, i.e., (𝑥0, 𝑦0, 𝑧0) are used 
instead; therefore, 
{⎧𝐹𝑥
}⎫
𝐹𝑦
𝐹𝑧⎭}⎬
⎩{⎨
=
𝑓 ̂
{⎧𝑥0 − 𝑥1
}⎫
𝑦0 − 𝑦1
𝑧0 − 𝑧1 ⎭}⎬
⎩{⎨
{⎧𝑛𝑥
}⎫
= 𝑓 ̂
𝑛𝑦
𝑛𝑧⎭}⎬
⎩{⎨
. 
(19.5)
The increment in the  element force is determined from the  user specified force-
force-displacement/velocity 
  Currently,  nine 
types  of 
displacement  relation. 
relationships may be specified: 
1. 
2. 
3. 
4. 
5. 
6. 
7. 
8. 
9. 
linear elastic; 
linear viscous; 
nonlinear elastic; 
nonlinear viscous; 
elasto-plastic with isotropic hardening; 
general nonlinear; 
linear viscoelastic. 
inelastic tension and compression only. 
muscle model. 
The force-displacement relations for these models are discussed in the following 
later. 
19.1  Orientation Vectors 
An orientation vector, 
{⎧𝑚1
}⎫
𝑚2
𝑚3⎭}⎬
⎩{⎨
can be defined to control the direction the spring acts.  If orientation vectors are used, it 
is  strongly  recommended  that  the  nodes  of  the  discrete  element  be  coincident  and 
𝐦 =
(19.6)
,
LS-DYNA Theory Manual 
Discrete Elements and Masses 
remain approximately so throughout the calculation.  If the spring or damper is of finite 
length,  rotational  constraints  will  appear  in  the  model  that  can  substantially  affect  the 
results.    If  finite  length  springs  are  needed  with  directional  vectors,  then  the  discrete 
beam elements, the type 6 beam, should be used with the coordinate system flagged for 
the finite length case. 
We will first consider the portion of the displacement that lies in the direction of 
the  vector.    The  displacement  of  the  spring  is  updated  based  on  the  change  of  length 
given by 
where  𝐼0  is  the  initial  length  in  the  direction  of  the  vector  and  lis  the  current  length 
given for a node to node spring by 
Δ𝐼 = 𝐼 − 𝐼0,
(19.7)
𝐼 = 𝑚1(𝑥2 − 𝑥1) + 𝑚2(𝑦2 − 𝑦1) + 𝑚3(𝑧2 − 𝑧1),
and for a node to ground spring by 
𝐼 = 𝑚1(𝑥0 − 𝑥1) + 𝑚2(𝑦0 − 𝑦1) + 𝑚3(𝑧0 − 𝑧1),
(19.8)
(19.9)
The  latter  case  is  not  intuitively  obvious  and  can  affect  the  sign  of  the  force  in 
unexpected  ways  if  the  user  is  not  familiar  with  the  relevant  equations.    The  nodal 
forces are then given by 
{⎧𝐹𝑥
}⎫
𝐹𝑦
𝐹𝑧⎭}⎬
⎩{⎨
{⎧𝑚1
}⎫
= 𝑓 ̂
𝑚2
𝑚3⎭}⎬
⎩{⎨
. 
(19.10)
The orientation vector can be either permanently fixed in space as defined in the 
input  or  acting  in  a  direction  determined  by  two  moving  nodes  which  must  not  be 
coincident  but  may  be  independent  of  the  nodes  of  the  spring.    In  the  latter  case,  we 
recompute the direction every cycle according to: 
𝑛 − 𝑥1
{⎧𝑥2
}⎫
𝑛 − 𝑦1
𝑦2
𝑛 ⎭}⎬
⎩{⎨
𝑛 − 𝑧1
𝑧2
{⎧𝑚1
}⎫
𝑚2
𝑚3⎭}⎬
⎩{⎨
In Equation (19.9) the superscript, 𝑛, refers to the orientation nodes.   
𝑙𝑛  
(19.11)
=
. 
For  the  case  where  we  consider  motion  in  the  plane  perpendicular  to  the 
orientation vector we consider only the displacements in the plane, Δ𝑙𝑝, given by, 
Δ𝐥𝑝 = Δ𝐥 − 𝐦(𝐦 ⋅ Δ𝐥).
(19.12)
We  update  the  displacement  of  the  spring  based  on  the  change  of  length  in  the  plane 
given by 
(19.13)
𝑝  is  the  initial  length  in  the  direction  of  the  vector  and  𝑙  is  the  current  length 
𝑝,
Δ𝑙𝑝 = 𝑙𝑝 − 𝑙0
where  𝑙0
given for a node to node spring by
Discrete Elements and Masses 
LS-DYNA Theory Manual 
𝑙𝑝 = 𝑚1
𝑝(𝑥2 − 𝑥1) + 𝑚2
𝑝(𝑦2 − 𝑦1) + 𝑚3
𝑝(𝑧2 − 𝑧1),
and for a node to ground spring by 
𝑙𝑝 = 𝑚1
𝑝(𝑥0 − 𝑥1) + 𝑚2
𝑝(𝑦0 − 𝑦1) + 𝑚3
𝑝(𝑧0 − 𝑧1),
where 
⎧𝑚1
{{
𝑚2
⎨
{{
𝑚3
⎩
⎫
}}
⎬
}}
⎭
=
𝑝 2
√Δ𝑙𝑥
𝑝 2
+ Δ𝑙𝑦
𝑝 2
+ Δ𝑙𝑧
⎧Δ𝑙𝑥
{{
Δ𝑙𝑦
⎨
{{
Δ𝑙𝑧
⎩
⎫
}}
⎬
}}
⎭
. 
After computing the displacements, the nodal forces are then given by 
{⎧𝐹𝑥
}⎫
𝐹𝑦
𝐹𝑧⎭}⎬
⎩{⎨
⎧𝑚1
{{
= 𝑓 ̂
𝑚2
⎨
{{
𝑚3
⎩
⎫
}}
⎬
}}
⎭
. 
(19.14)
(19.15)
(19.16)
(19.17)
19.2  Dynamic Magnification “Strain Rate” Effects 
To account for “strain rate” effects, we have a simple method of scaling the forces 
based  on  the  relative  velocities  that  applies  to  all  springs.    The  forces  computed  from 
the  spring  elements  are  assumed  to  be  the  static  values  and  are  scaled  by  an 
amplification factor to obtain the dynamic value: 
𝐹dynamic = (1. + 𝑘𝑑
𝑉0
) 𝐹static,
(19.18)
where 
𝑘𝑑 = is a user defined input value 
𝑉 = absolute relative velocity  
𝑉0 = dynamic test velocity 
For example, if it is known that a component shows a dynamic crush force at 15 
m/s equal to 2.5 times the static crush force, use 𝑘𝑑 = 1.5 and 𝑉0 = 15. 
19.3  Deflection Limits in Tension and Compression 
The deflection limit in compression and tension is restricted in its application to 
no more than one spring per node subject to this limit, and to deformable bodies only.  
For example in the former case, if three spring are in series either the center spring or 
the  two  end  springs  may  be  subject  to  a  limit  but  not  all  three.    When  the  limiting
LS-DYNA Theory Manual 
Discrete Elements and Masses 
deflection  is  reached  momentum  conservation  calculations  are  performed  and  a 
common acceleration is computed: 
1 + 𝑓 ̂
𝑓 ̂
𝑚1 + 𝑚2
An error termination will occur if a rigid body node is used in a spring definition where 
compression is limited. 
𝑎 ̂common =
(19.19)
.
19.4  Linear Elastic or Linear Viscous 
These  discrete  elements  have  the  simplest  force-displacement  relations.    The 
linear elastic discrete element has a force-displacement relation of the form 
𝑓 ̂ = 𝐾Δ𝑙,
(19.20)
where  𝐾  is  the  element’s  stiffness  and  Δ𝑙  is  the  change  in  length  of  the  element.    The 
linear viscous element has a similar force-velocity (rate of displacement) relation: 
where 𝐶 is a viscous damping parameter and Δ𝑡 is the time step increment. 
𝑓 ̂ = 𝐶
Δ𝑙
Δ𝑡
.
(19.21)
19.5  Nonlinear Elastic or Nonlinear Viscous 
These  discrete  elements  use  piecewise  force-displacement  or  force-relative 
velocity  relations.    The  nonlinear  elastic  discrete  element  has  a  tabulated  force-
displacement relation of the form 
𝑓 ̂ = 𝐾Δ𝑙,
(19.22)
where 𝐾(Δ𝑙) is the tabulated force that depends on the total change in the length of the 
element  (Figure  19.1)    The  nonlinear  viscous  element  has  a  similar  tabulated  force-
relative  velocity relation: 
𝑓 ̂ = 𝐶
Δ𝑙
Δ𝑡
,
(19.23)
where  𝐶(Δ𝑙
element’s length.  Nonlinear discrete elements unload along the loading paths. 
Δ𝑡)  is  the  viscous  damping  force  that  depends  on  the  rate  of  change  of  the 
If  the  spring  element  is  initially  of  zero  length  and  if  no  orientation  vectors  are 
used then only the tensile part of the stress strain curve needs to be defined.  However,
Discrete Elements and Masses 
LS-DYNA Theory Manual 
Nolinear Elastic/Viscous
Displacement/Velocity
Figure  19.1.    Piecewise  linear  force-displacement  curve  for  nonlinear  elastic
discrete element. 
if the spring element is initially of finite length then the curve must be defined in both 
the positive and negative quadrants.   
19.6  Elasto-Plastic with Isotropic Hardening 
The elasto-plastic discrete element has a bilinear force-displacement relationship 
that is specified by the elastic stiffness, a tangent stiffness and a yield force (Figure 19.2).  
This discrete element uses the elastic stiffness model for unloading until the yield force 
is exceeded during unloading.  The yield force is updated to track its maximum value 
which  is  equivalent  to  an  isotropic  hardening  model.    The  force-displacement  relation 
during loading may be written as 
𝑓 ̂ = 𝐹𝑦 (1 −
𝐾𝑡
) + 𝐾𝑡Δ𝑙,
(19.24)
where 𝐹𝑦 is the yield force and 𝐾𝑡 is the tangent stiffness. 
19.7  General Nonlinear 
The  general  nonlinear  discrete  element  allows  the  user  to  specify  independent 
and nonsymmetrical piecewise linear loading and unloading paths (Figure 19.3(a)).
LS-DYNA Theory Manual 
Discrete Elements and Masses 
Elsto-Plastic with
Isotropic Hardening
ET
FY
Elasto-Plastic Unloading
Figure  19.2.    Loading  and  unloading  force-displacement  curves  for  elasto-
plastic discrete element. 
Displacement
This element combines the features of the above-described nonlinear elastic and 
elasto-plastic discrete elements by allowing the user to specify independent initial yield 
forces in tension (FYT) and in compression (FYC).  If the discrete element force remains 
between  these  initial  yield  values,  the  element  unloads  along the  loading  path  (Figure 
19.3(b)).  This corresponds to the nonlinear elastic discrete element. 
However, if the discrete element force exceeds either of these initial yield values, 
the  specified  unloading  curve  is  used  for  subsequent  unloading.    Additionally,  the 
initial  loading  and  unloading  curves  are  allowed  to  move  in  the  force-displacement 
space  by  specifying  a  mixed  hardening  parameter  𝛽,  where  𝛽 = 0  corresponds  to 
kinematic  hardening  (Figure  19.3(c))  and  𝛽 = 0  𝛽 = 1  corresponds  to  isotropic 
hardening (Figure 19.3(d)). 
19.8  Linear Visco-Elastic 
The  linear  viscoelastic  discrete  element  [Schwer,  Cheva,  and  Hallquist  1991] 
allows the user to model discrete components that are characterized by force relaxation 
or  displacement  creep  behavior.    The  element’s  variable  stiffness  is  defined  by  three 
parameters and has the form 
𝐾(𝑡) = 𝐾∞ + (𝐾0 − 𝐾∞)𝑒−𝛽𝑡,
(19.25)
Discrete Elements and Masses 
LS-DYNA Theory Manual 
loading
curve
options
β>0
β=0
yt - F
yc
Fyt
Fyc
β>0
β=0
unloading curve
kinematic hardening  β<1
isotropic hardening  β=1
force
force
Fyt-Fyc
F2
F2
F1
Figure  19.3.    Loading  and  unloading  force  displacement  curves  for  general
nonlinear discrete element. 
where 𝐾∞ is the long duration stiffness, 𝐾0 is the short time stiffness, and 𝛽 is a decay 
parameter that controls the rate at which the stiffness transitions between the short and 
long duration stiffness (Figure 16.4). 
This  model  corresponds  to  a  three-parameter  Maxwell  model    which  consists  of  a  spring  and  damper  in  series  connected  to  another 
spring in parallel.  Although this discrete element behavior could be built up using the 
above- described linear elastic and linear viscous discrete elements, such a model would 
also require the user to specify the nodal mass at the connection of the series spring and 
damper.    This  mass  introduces  a  fourth  parameter  which  would  further  complicate 
fitting the model to experimental data.
LS-DYNA Theory Manual 
Discrete Elements and Masses 
Log K0
)
(
Log K∞
K∞
Visco-Elastic
K0-K∞
1/β
Log t
Figure 19.4.  Typical stiffness relaxation curve used for the viscoelastic discrete
element. 
19.9  Muscle Model 
This  is  Material  Type  15  for  discrete  springs  and  dampers.    This  material  is  a 
Hill-type  muscle  model  with  activation.    It  is  for  use  with  discrete  elements.    The  LS-
DYNA implementation is due to Dr.  J.A. Weiss. 
L0 
VMAX 
SV 
Initial muscle length, Lo. 
Maximum CE shortening velocity, Vmax. 
Scale factor, Sv, for Vmax vs.  active state. 
A 
Activation level vs.  time function. 
LT.0: absolute value gives load curve ID 
GE.0: constant value of 1.0 is used 
LT.0: absolute value gives load curve ID 
GE.0: constant value of A is used 
FMAX Peak isometric force, Fmax. 
TL  Active tension vs.  length function. 
LT.0: absolute value gives load curve ID 
GE.0: constant value of 1.0 is used
Discrete Elements and Masses 
LS-DYNA Theory Manual 
FM
FCE
FPE
a(t)
SEE
LM
vM
CE
LM
PE
FM
Figure 19.5.  Discrete model for muscle contraction dynamics, based on a Hill-
type representation.  The total force is the sum of passive force FPE and active 
force  FCE.    The  passive  element  (PE)  represents  energy  storage  from  muscle
elasticity, while the contractile element (CE) represents force generation by the
muscle.    The  series  elastic  element  (SEE),  shown  in  dashed  lines,  is  often 
neglected  when  a  series  tendon  compliance  is  included.    Here,  a(t)  is  the
activation  level,  LM  is  the  length  of  the  muscle,  and  vM  is  the  shortening
velocity of the muscle. 
TV  Active tension vs.  velocity function. 
FPE  Force vs.  length function, Fpe, for parallel elastic element. 
LT.0: absolute value gives load curve ID 
GE.0: constant value of 1.0 is used 
LT.0: absolute value gives load curve ID 
EQ.0: exponential function is used  
GT.0: constant value of 0.0 is used 
Relative length when Fpe reaches Fmax.  Required if Fpe = 0 above. 
LMAX 
KSH  Constant, Ksh,  governing  the  exponential  rise  of  Fpe.    Required  if  Fpe = 0 
above. 
The  material  behavior  of  the  muscle  model  is  adapted  from  the  original  model 
proposed by Hill (1938).  Reviews of this model and extensions can be found in Winters 
(1990) and Zajac (1989).  The most basic Hill-type muscle model consists of a contractile 
element  (CE)  and  a  parallel  elastic  element  (PE)  (Figure  19.5).    An  additional  series 
elastic  element  (SEE)  can  be  added  to  represent  tendon  compliance.    The  main 
assumptions of the Hill model are that the contractile element is entirely stress free and 
freely  distensible  in  the  resting  state,  and  is  described  exactly  by  Hill’s  equation  (or 
some  variation).    When  the  muscle  is  activated,  the  series  and  parallel  elements  are 
elastic, and the whole muscle is a simple combination of identical sarcomeres in series 
and  parallel.    The  main  criticism  of  Hill’s  model  is  that  the  division  of  forces  between 
the  parallel  elements  and  the  division  of  extensions  between  the  series  elements  is 
arbitrary,  and  cannot  be  made  without  introducing  auxiliary  hypotheses.    However, 
these criticisms apply to any discrete element model.  Despite these limitations, the Hill 
model  has  become  extremely  useful  for  modeling  musculoskeletal  dynamics,  as 
illustrated by its widespread use today. 
When  the  contractile  element  (CE)  of  the  Hill  model  is  inactive,  the  entire 
resistance to elongation is provided by the PE element and the tendon load-elongation
LS-DYNA Theory Manual 
Discrete Elements and Masses 
behavior.    As  activation  is  increased,  force  then  passes  through  the  CE  side  of  the 
parallel  Hill  model,  providing  the  contractile  dynamics.    The  original  Hill  model 
accommodated  only  full  activation  -  this  limitation  is  circumvented  in  the  present 
implementation  by  using  the  modification  suggested  by  Winters  (1990).    The  main 
features of his approach were to realize that the CE force-velocity input force equals the 
CE  tension-length  output  force.    This  yields  a  three-dimensional  curve  to  describe  the 
force-velocity-length relationship of the CE.  If the force-velocity y-intercept scales with 
activation,  then  given  the  activation,  length  and  velocity,  the  CE  force  can  be 
determined. 
Without the SEE, the total force in the muscle FM is the sum of the force in the 
CE and the PE because they are in parallel: 
𝐹M = 𝐹PE + 𝐹CE.
(19.26)
The  relationships  defining  the  force  generated  by  the  CE  and  PE  as  a  function  of  LM, 
VM and 𝑎(𝑡) are often scaled by 𝐹max, the peak isometric force (p.  80, Winters 1990), L0, 
the initial length of the muscle (p.  81, Winters 1990), and 𝑉max, the maximum unloaded 
CE  shortening  velocity  (p.    80,  Winters  1990).    From  these,  dimensionless  length  and 
velocity can be defined: 
𝐿 =
𝑉 =
𝐿M
𝐿o
, 
𝑉M
𝑉max ∗ 𝑆V(𝑎(t))
.
(19.27)
Here, 𝑆V scales the maximum CE shortening velocity 𝑉max and changes with activation 
level 𝑎(𝑡). This has been suggested by several researchers, i.e. Winters and Stark [1985].  
The activation level specifies the level of muscle stimulation as a function of time.  Both 
have  values  between  0  and  1.  The  functions  𝑆V(𝑎(𝑡))  and  𝑎(𝑡)  are  specified  via  load 
curves  in  LS-DYNA,  or  default  values  of 𝑆V = 1  and  𝑎(𝑡) = 0  are  used.    Note  that  L  is 
always positive and that 𝑉 is positive for lengthening and negative for shortening. 
The relationship between FCE, V and L was proposed by Bahler et al.  [1967].  A 
three-dimensional relationship between these quantities is now considered standard for 
computer  implementations  of  Hill-type  muscle  models  [i.e.,  eqn  5.16,  p.  81,  Winters 
1990].  It can be written in dimensionless form as: 
𝐹CE = 𝑎(𝑡) ∗ 𝐹max ∗ 𝑓TL(𝐿) ∗ 𝑓TV(𝑉),
(19.28)
The  force  in  the  parallel  elastic  element  FPE  is  determined  directly  from  the  current 
length of the muscle using an exponential relationship [eqn 5.5, p. 73, Winters 1990]: 
𝑓PE =
𝐹PE
𝐹MAX
= 0
𝐿 ≤ 1
𝑓PE =
𝐹PE
𝐹MAX
=
exp(𝐾sh) − 1
[exp
⎜⎛ 𝐾sh
𝐿max
⎝
(L − 1)
⎟⎞ − 1] 𝐿 > 1
⎠
(19.29)
Discrete Elements and Masses 
LS-DYNA Theory Manual 
Figure 19.6.  Typical normalized tension-length (TL) and tension-velocity (TV)
curves for skeletal muscle. 
For computation of the total force developed in the muscle FM, the functions for 
the tension-length 𝑓TLand force-velocity 𝑓TV relationships used in the Hill element must 
be  defined.    These  relationships  have  been  available  for  over  50  years,  but  have  been 
refined  to  allow  for  behavior  such  as  active  lengthening.    The  active  tension-length 
curve  𝑓TL  describes  the  fact  that  isometric  muscle  force  development  is  a  function  of 
length, with the maximum force occurring at an optimal length.  According to Winters, 
this  optimal  length  is  typically  around  𝐿 = 1.05,  and  the  force  drops  off  for  shorter  or 
longer  lengths,  approaching  zero  force  for  𝐿 = 0.4  and  𝐿 = 1.5.  Thus  the  curve  has  a 
bell-shape.    Because  of  the  variability  in  this  curve  between  muscles,  the  user  must 
specify  the  function  𝑓TL  via  a  load  curve,  specifying  pairs  of  points  representing  the 
normalized force (with values between 0 and 1) and normalized length 𝐿 (Figure 19.6). 
The  active  tension-velocity  relationship  𝑓TV  used  in  the  muscle  model  is  mainly 
due to the original work of Hill.  Note that the dimensionless velocity V is used.  When 
V = 0,  the  normalized  tension  is  typically  chosen  to  have  a  value  of  1.0.    When  V  is 
greater  than  or  equal  to  0,  muscle  lengthening  occurs.    As  V  increases,  the  function  is 
typically  designed  so  that  the  force  increases  from  a  value  of  1.0  and  asymptotes 
towards a value near 1.4.  When V is less than zero, muscle shortening occurs and the 
classic Hill equation hyperbola is used to drop the normalized tension to 0 (Figure 16.6).  
The  user  must  specify  the  function  𝑓TV    via  a  load  curve,  specifying  pairs  of  points 
representing  the  normalized  tension  (with  values  between  0  and  1)  and  normalized 
velocity V.
LS-DYNA Theory Manual 
Discrete Elements and Masses 
19.10  Seat Belt Material 
The seat belt capability reported here was developed by Walker and co-workers 
[Walker  and  Dallard  1991,  Strut,  Walker,  et al.,  1991]  and  this  section  excerpted  from 
their  documentation.    Each  belt  material  defines  stretch  characteristics  and  mass 
properties for a set of belt elements.  The user enters a load curve for loading, the points 
of which are (Strain, Force).  Strain is defined as engineering strain, i.e. 
Strain =
current   length
initial  length
− 1.
(19.30)
Another  similar  curve  is  entered  to  describe  the  unloading  behavior.    Both 
loadcurves  should  start  at  the origin  (0,0)  and  contain  positive  force  and  strain  values 
only.  The belt material is tension only with zero forces being generated whenever the 
strain  becomes  negative.    The  first  non-zero  point  on  the  loading  curve  defines  the 
initial yield point of the material.  On  unloading, the unloading  curve is shifted along 
the  strain  axis  until  it  crosses  the  loading  curve  at  the  ‘yield’  point  from  which 
unloading commences.  If the initial yield has not yet been exceeded or if the origin of 
the  (shifted)  unloading  curve  is  at  negative  strain,  the  original  loading  curves  will  be 
used for both loading and unloading.  If the strain is less than the strain at the origin of 
the unloading curve, the belt is slack and no force is generated.  Otherwise, forces will 
then be determined by the unloading curve for unloading and reloading until the strain 
again exceeds yield after which the loading curves will again be used. 
A  small  amount  of  damping  is  automatically  included.    This  reduces  high 
frequency  oscillation,  but,  with  realistic  force-strain  input  characteristics  and  loading 
rates,  does  not  significantly  alter  the  overall  forces-strain  performance.    The  damping 
forced opposes the relative motion of the nodes and is limited by stability: 
𝐷 =
. 1 × mass × relative  velocity
timestep  size
.
(19.31)
In  addition,  the  magnitude  of  the  damping  forces  is  limited  to  one  tenth  of  the 
force  calculated  from  the  forces-strain  relationship  and  is  zero  when  the  belt  is  slack.  
Damping forces are not applied to elements attached to sliprings and retractors. 
The user inputs a mass per unit length that is used to calculate nodal masses on 
initialization. 
A  ‘minimum  length’  is  also  input.    This  controls  the  shortest  length  allowed  in 
any element and determines when an element passes through sliprings or are absorbed 
into the retractors.  One tenth of a typical initial element length is usually a good choice.
Discrete Elements and Masses 
LS-DYNA Theory Manual 
19.11  Seat Belt Elements 
Belt  elements  are  single  degree  of  freedom  elements  connecting  two  nodes  and 
are treated in a manner similar to the spring elements.  When the strain in an element is 
positive (i.e., the current length is greater then the unstretched length), a tension force is 
calculated from the material characteristics and is applied along the current axis of the 
element to oppose further stretching.  The unstretched length of the belt is taken as the 
initial  distance  between  the  two  nodes  defining  the  position  of  the  element  plus  the 
initial  slack  length.    At  the  beginning  of  the  calculation  the  seatbelt  elements  can  be 
obtained within a retractor. 
19.12  Sliprings 
Sliprings are defined in the LS-DYNA input by giving a slipring ID and element 
ID’s for two elements who share a node which is coincident with the slipring node.  The 
slipring node may not be attached to any belt elements. 
Sliprings  allow  continuous  sliding  of  a  belt  through  a  sharp  change  of  angle.  
Two elements (1 and 2 in Figure 19.7) meet at the slipring.  Node B in the belt material 
remains  attached  to  the  slipring  node,  but  belt  material  (in  the  form  of  unstretched 
length) is passed from element 1 to element 2 to achieve slip.  The amount of slip at each 
timestep is calculated from the ratio of forces in elements 1 and 2.  The ratio of forces is 
determined  by  the  relative  angle  between  elements  1  and  2  and  the  coefficient  of 
friction,  𝜇.    The  tension  in  the  belts  is  taken  as  T1  and  T2,  where  T2  is  on  the  high-
tension side and T1 is the force on the low-tension side.  Thus if T2 is sufficiently close 
to T1 no slip occurs; otherwise, slip is just sufficient to reduce the ratio T2⁄T1 to 𝑒𝜇𝜃.  No 
slip occurs if both elements are slack.  The out-of-balance force at node B is reacted on 
the slipring node; the motion of node B follows that of slipring node. 
If, due to slip through the slipring, the unstretched length of an element becomes 
less  than  the  minimum  length  (as  entered  on  the  belt  material  card),  the  belt  is 
remeshed locally:   the short element passes through the slipring and reappears on the 
other side .  The new unstretched length of e1 is 1.1 × minimum length.  
Force  and  strain  in  e2  and  e3  are  unchanged;  force  and  strain  in  e1  are  now  equal  to 
those in e2.  Subsequent slip will pass material from e3 to e1.  This process can continue 
with several elements passing in turn through the slipring.  
To define a slipring, the user identifies the two belt elements which meet at the 
slipring, the friction coefficient, and the slipring node.  The two elements must have a 
common  node  coincident  with  the  slipring  node.    No  attempt  should  be  made  to 
restrain or constrain the common node for its motion will automatically be constrained 
to  follow  the  slipring  node.    Typically,  the  slipring  node  is  part  of  the  vehicle  body
LS-DYNA Theory Manual 
Discrete Elements and Masses 
Slip ring
Element 2
Element 1
Element 1
Element 3
Element 2
Element 3
Before
After
Figure 19.7.  Elements passing through slipring. 
structure and, therefore, belt elements should not be connected to this node directly, but 
any other feature can be attached, including rigid bodies. 
19.13  Retractors 
Retractors are defined by giving a node, the “retractor node” and an element ID 
of  an  element  outside  the  retractor  but  with  one  node  that  is  coincident  with  the 
retractor  node.    Also  sensor  ID’s  must  be  defined  for  up  to  four  sensors  which  can 
activate the seatbelt. 
Retractors allow belt material to be paid out into a belt element, and they operate 
in one of two regimes: unlocked when the belt material is paid out or reeled in under 
constant tension and locked when a user defined force-pullout relationship applies. 
The  retractor  is  initially  unlocked,  and  the  following  sequence  of  events  must 
occur for it to become locked: 
•  Any  one  of  up  to  four  sensors  must  be  triggered.    (The  sensors  are  described 
below). 
•  Then a user-defined time delay occurs. 
•  Then a user-defined length of belt must be payed out (optional). 
•  Then the retractor locks. 
and once locked, it remains locked.
Discrete Elements and Masses 
LS-DYNA Theory Manual 
In the unlocked regime, the retractor attempts to apply a constant tension to the 
belt.    This  feature  allows  an  initial  tightening  of  the  belt,  and  takes  up  any  slack 
whenever it occurs.  The tension value is taken from the first point on the force-pullout 
load curve.  The maximum rate of pull out or pull in is given by 0.01 × fed length per 
time step.  Because of this, the constant tension value is not always achieved. 
In the locked regime, a user-defined curve describes the relationship between the 
force in the attached element and the amount of belt material paid out.  If the tension in 
the belt subsequently relaxes, a different user-defined curve applies for unloading.  The 
unloading curve is followed until the minimum tension is reached. 
The curves are defined in terms of initial length of belt.  For example, if a belt is 
marked at 10mm intervals and then wound  onto a retractor, and the force required to 
make  each  mark  emerge  from  the  (locked)  retractor  is  recorded,  the  curves  used  for 
input would be as follows: 
0 Minimum tension (should be > zero) 
10 mm Force to emergence of first mark 
20 mm Force to emergence of second mark 
.. 
.. 
.. 
Pyrotechnic pretensions may be defined which cause the retractor to pull in the 
belt  at  a  predetermined  rate.    This  overrides  the  retractor  force-pullout  relationship 
from the moment when the pretensioner activates. 
If  desired,  belt  elements  may  be  defined which  are  initially  inside  the  retractor.  
These  will  emerge  as  belt  material  is  paid  out,  and  may  return  into  the  retractor  if 
sufficient material is reeled in during unloading.  
Elements  e2,  e3  and  e4  are  initially  inside  the  retractor,  which  is  paying  out 
material into element e1.  When the retractor has fed Lcrit into e1, where: 
Lcrit = fed length − 1.1 × minimum length
(19.32)
Here,  minimum  length  is  defined  on  belt  material  input,  and  fed  length  is  defined  on 
retractor input.  
element  e2  emerges  with  an  unstretched  length  of  1.1  ×  minimum  length;  the 
unstretched length of element e1 is reduced by the same amount.  The force and strain 
in e1 are unchanged; in e2, they are set equal to those in e1.  The retractor now pays out 
material into e2.
LS-DYNA Theory Manual 
Discrete Elements and Masses 
If no elements are inside the retractor, e2 can continue to extend as more material 
is fed into it. 
As  the  retractor  pulls  in  the  belt  (for  example,  during  initial  tightening),  if  the 
unstretched  length  of  the  mouth  element  becomes  less  than  the  minimum  length,  the 
element is taken into the retractor. 
To define a retractor, the user enters the retractor node, the ‘mouth’ element (into 
which  belt  material  will  be  fed,  e1  in  Figure  19.8,  up  to  4  sensors  which  can  trigger 
unlocking, a time delay, a payout delay (optional), load and unload curve numbers, and 
the fed length.  The retractor node is typically part of the vehicle stricture; belt elements 
should  not  be  connected  to  this  node  directly,  but  any  other  feature  can  be  attached 
including  rigid  bodies.    The  mouth  element  should  have  a  node  coincident  with  the 
retractor but should not be inside the retractor.  The fed length would typically be set 
either  to  a  typical  element  initial  length,  for  the  distance  between  painted  marks  on  a 
real belt for comparisons with high-speed film.  The fed length should be at least three 
times the minimum length. 
If there are elements initially inside the retractor (e2, e3 and e4 in the Figure) they 
should not be referred to on the retractor input, but the retractor should be identified on 
the  element  input  for  these  elements.    Their  nodes  should  all  be  coincident  with  the 
retractor  node  and  should  not  be  restrained  or  constrained.    Initial  slack  will 
automatically  be  set  to  1.1  ×  minimum  length  for  these  elements;  this  overrides  any 
user-defined value.
Discrete Elements and Masses 
LS-DYNA Theory Manual 
Before
Element 1
Element 1
Element 2
Element 4
Element 3
Element 2
After
Element 3
Element 4
Element 4
Element 4
All nodes within this area
are coincident
Figure 19.8.  Elements in a retractor. 
Weblockers  can  be  included  within  the  retractor  representation  simply  by 
entering  a  ‘locking  up’  characteristic  in  the  force  pullout  curve,  see  Figure  19.9.    The 
final section can be very steep (but must have a finite slope). 
with weblockers
without weblockers
Pullout
Figure 19.9.  Retractor force pull characteristics.
LS-DYNA Theory Manual 
Discrete Elements and Masses 
19.14  Sensors 
Sensors are used to trigger locking of retractors and activate pretensioners.  Four 
types of sensor are available which trigger according to the following criteria: 
Type 1–When the magnitude of x-, y-, or z- acceleration of a given node has remained 
above  a  given  level  continuously  for  a  given  time,  the  sensor  triggers.    This  does  not 
work with nodes on rigid bodies. 
Type 2–When the rate of belt payout from a given retractor has remained above a given 
level continuously for a given time, the sensor triggers. 
Type 3–The sensor triggers at a given time. 
Type  4–The  sensor  triggers  when  the  distance  between  two  nodes  exceeds  a  given 
maximum or becomes less than a given minimum.  This type of sensor is intended for 
use with an explicit mas/spring representation of the sensor mechanism. 
By  default,  the  sensors  are  inactive  during  dynamic  relaxation.    This  allows 
initial tightening of the belt and positioning of the occupant on the seat without locking 
the retractor or firing any pretensioners.  However, a flag can be set in the sensor input 
to make the sensors active during the dynamic relaxation phase. 
19.15  Pretensioners 
Pretensioners allow modeling of three types of active devices which tighten the 
belt during the initial stages of a crash.  The first type represents a pyrotechnic device 
which spins the spool of a retractor, causing the belt to be reeled in.  The user defines a 
pull-in versus time curve which applies once the pretensioner activates.  The remaining 
types  represents  preloaded  springs  or  torsion  bars  which  move  the  buckle  when 
released.    The  pretensioner  is  associated  with  any  type  of  spring  element  including 
rotational.    Note  that  the  preloaded  spring,  locking  spring  and  any  restraints  on  the 
motion  of  the  associated  nodes  are  defined  in  the  normal  way;  the  action  of  the 
pretensioner is merely to cancel the force in one spring until (or after) it fires.  With the 
second  type,  the  force  in  the  spring  element  is  cancelled  out  until  the  pretensioner  is 
activated.  In this case the spring in question is normally a stiff, linear spring which acts 
as  a  locking  mechanism,  preventing  motion  of  the  seat  belt  buckle  relative  to  the 
vehicle.    A  preloaded  spring  is  defined  in  parallel  with  the  locking  spring.    This  type 
avoids  the  problem  of  the  buckle  being  free  to  ‘drift’  before  the  pretensioner  is 
activated. 
To activate the pretensioner the following sequence of events must occur:
Discrete Elements and Masses 
LS-DYNA Theory Manual 
1. Any one of up to four sensors must be triggered. 
2. Then a user-defined time delay occurs. 
3. Then the pretensioner acts. 
19.16  Accelerometers 
The accelerometer is defined by three nodes in a rigid body which defines a triad 
to measure the accelerations in a local system.  The presence of the accelerometer means 
that the accelerations and velocities of node 1 will be output to all output files in local 
instead of global coordinates. 
The local coordinate system is defined by the three nodes as follows: 
•  local 𝐱 from node 1 to node 2 
•  local 𝐳 perpendicular to the plane containing nodes, 1, 2, and 3 (𝐳 = 𝐱 × 𝐚), where 
𝐚 is from node 1 to node 3). 
•  local 𝐲 = 𝐱 × 𝐳 
The  three  nodes  should  all  be  part  of  the  same  rigid  body.    The  local  axis  then 
rotates with the body.
LS-DYNA Theory Manual 
Simplified Arbitrary Lagrangian-Eulerian 
20    
Simplified Arbitrary Lagrangian-
Eulerian 
Arbitrary  Lagrangian-Eulerian  (ALE)  formulations  may  be  thought  of  as 
algorithms that perform automatic rezoning.  Users perform manual rezoning by  
1. 
2. 
Stopping the calculation when the mesh is distorted,  
Smoothing the mesh,  
3.  Remapping the solution from the distorted mesh to the smooth mesh. 
An ALE formulation consists of a Lagrangian time step followed by a “remap” or 
“advection”  step.    The  advection  step  performs  an  incremental  rezone,  where 
“incremental” refers to the fact that the positions of the nodes are moved only a small 
fraction  of  the  characteristic  lengths  of  the  surrounding  elements.    Unlike  a  manual 
rezone, the topology of the mesh is fixed in an ALE calculation.  An ALE calculation can 
be  interrupted  like  an  ordinary  Lagrangian  calculation  and  a  manual  rezone  can  be 
performed if an entirely new mesh is necessary to continue the calculation. 
The  accuracy  of  an  ALE  calculation  is  often  superior  to  the  accuracy  of  a 
manually  rezoned  calculation  because  the  algorithm  used  to  remap  the  solution  from 
the distorted to the undistorted mesh is second order accurate for the ALE formulation 
while the algorithm for the manual rezone is only first order accurate. 
In  theory,  an  ALE  formulation  contains  the  Eulerian  formulation  as  a  subset.  
Eulerian  codes  can  have  more  than  one  material  in  each  element,  but  most  ALE 
implementations  are  simplified  ALE  formulations  which  permit  only  a  single  material 
in each element.  The primary advantage of a simplified formulation is its reduced cost 
per time step.  When elements with more than one material are permitted, the number 
and types of materials present in an element can change dynamically.  Additional data
Simplified Arbitrary Lagrangian-Eulerian 
LS-DYNA Theory Manual 
is necessary to specify the materials in each element and the data must be updated by 
the remap algorithms. 
The  range  of  problems  that  can  be  solved  with  an  ALE  formulation  is  a  direct 
function  of  the  sophistication  of  the  algorithms  for  smoothing  the  mesh.    Early  ALE 
codes  were  not  very  successful  largely  because  of  their  primitive  algorithms  for 
smoothing the mesh.  In simplified ALE formulations, most of the difficulties with the 
mesh  are  associated  with  the  nodes  on  the  material  boundaries.    If  the  material 
boundaries are purely Lagrangian, i.e., the boundary nodes move with the material at 
all  times,  no  smooth  mesh  maybe  possible  and  the  calculation  will  terminate.    The 
algorithms for maintaining a smooth boundary mesh are therefore as important to the 
robustness of the calculations as the algorithms for the mesh interior.   
The cost of the advection step per element is usually much larger than the cost of 
the Lagrangian step.  Most of the time in the advection step is spent in calculating the 
material transported between the adjacent elements, and only a small part of it is spent 
on  calculating  how  and  where  the  mesh  should  be  adjusted.    Second  order  accurate 
monotonic  advection  algorithms  are  used  in  LS-DYNA  despite  their  high  cost  per 
element because their superior coarse mesh accuracy which allows the calculation to be 
performed  with  far  fewer  elements  than  would  be  possible  with  a  cheaper  first  order 
accurate algorithm. 
The  second  order  transport  accuracy  is  important  since  errors  in  the  transport 
calculations generally smooth out the solution and reduce the peak values in the history 
variables.    Monotonic  advection  algorithms  are  constructed  to  prevent  the  transport 
calculations from creating new minimum or maximum values for the solution variables.  
They were first developed for the solution of the Navier Stokes equations to eliminate 
the  spurious  oscillations  that  appeared  around  the  shock  fronts.   Although  monotonic 
algorithms  are  more  diffusive  than  algorithms  that  are  not  monotonic,  they  must  be 
used  for  stability  in  general  purpose  codes.    Many  constitutive  models  have  history 
variables that have limited ranges, and if their values are allowed to fall outside of their 
allowable  ranges,  the  constitutive  models  are  undefined.    Examples  include  explosive 
models,  which  require  the  burn  fraction  to  be  between  zero  and  one,  and  many 
elastoplasticity models, such as those with power law hardening, which require a non-
negative plastic strain. 
The overall flow of an ALE time step is: 
1. 
2. 
Perform a Lagrangian time step. 
Perform an advection step. 
a)  Decide which nodes to move. 
b)  Move the boundary nodes.
LS-DYNA Theory Manual 
Simplified Arbitrary Lagrangian-Eulerian 
c)  Move the interior nodes. 
d)  Calculate the transport of the element-centered variables. 
e)  Calculate the momentum transport and update the velocity. 
Each  element  solution  variable  must  be  transported.    The  total  number  of 
solution  variables,  including  the  velocity,  is  at  least  six  and  depends  on  the  material 
models.  For elements that are modeled with an equation of state, only the density, the 
internal  energy,  and  the  shock  viscosity  are  transported.    When  the  elements  have 
strength,  the  six  components  of  the  stress  tensor  and  the  plastic  strain  must  also  be 
advected,  for  a  total  of  ten  solution  variables.    Kinematic  hardening,  if  it  is  used, 
introduces another five solution variables, for a total of fifteen.  
The  nodal  velocities  add  an  extra  three  solution  variables  that  must  be 
transported,  and  they  must  be  advected  separately  from  the  other  solution  variables 
because  they  are  centered  at  the  nodes  and  not  in  the  elements.    In  addition,  the 
momentum must be conserved, and it is a product of the node-centered velocity and the 
element-centered density.  This imposes a constraint on how the momentum transport 
is  performed  that  is  unique  to  the  velocity  field.    A  detailed  consideration  of  the 
difficulties associated with the transport of momentum is deferred until later. 
Perhaps the simplest strategy for minimizing the cost of the ALE calculations is 
to  perform them  only every  few  time  steps.   The  cost  of  an  advection  step  is  typically 
two to five times the cost of the Lagrangian time step.  By performing the advection step 
only every ten steps, the cost of an ALE calculation can often be reduced by a factor of 
three without adversely affecting the time step size.  In general, it is not worthwhile to 
advect  an  element  unless  at  least  twenty  percent  of  its  volume  will  be  transported 
because  the  gain  in  the  time  step  size  will  not  offset  the  cost  of  the  advection 
calculations.  
20.1  Mesh Smoothing Algorithms 
The algorithms for moving the mesh relative to the material control the range of 
the  problems  that  can  be  solved  by  an  ALE  formulation.    The  equipotential  method 
which  is  used  in  LS-DYNA  was  developed  by  Winslow  [1990]  and  is  also  used  in  the 
DYNA2D  ALE  code  [Winslow  1963].    It,  and  its  extensions,  have  proven  to  be  very 
successful  in  a  wide  variety  of  problems.    The  following  is  extracted  from  reports 
prepared by Alan Winslow for LSTC.
Simplified Arbitrary Lagrangian-Eulerian 
LS-DYNA Theory Manual 
20.1.1  Equipotential Smoothing of Interior Nodes 
“Equipotential”  zoning  [Winslow,  1963]  is  a  method  of  making  a  structured 
mesh for finite difference or finite element calculations by using the solutions of Laplace 
equations  (later  extended  to  Poisson  equations)  as  the  mesh  lines.    The  same  method 
can  be  used  to  smooth  selected  points  in  an  unstructured  three-dimensional  mesh 
provided that it is at least locally structured.  This chapter presents a derivation of the 
three-dimensional equipotential zoning equations, taken from the references, and gives 
their  finite  difference  equivalents  in  a  form  ready  to  be  used  for  smoothing  interior 
points.  We begin by reviewing the well-known two-dimensional zoning equations, and 
then discuss their extension to three dimensions. 
In two dimensions we define curvilinear coordinates 𝜉  𝜂 which satisfy Laplace’s 
equation:  
∇2𝜉 = 0,
∇2𝜂 = 0.
(20.1.1a)
(1.1.1b)
We  solve  Equations  (1.1.1b)  for  the  coordinates  𝑥(𝜉 , 𝜂)  and  𝑦(𝜉 , 𝜂)  of  the  mesh 
lines:  that  is,  we  invert  them  so  that  the  geometric  coordinates  𝑥, 𝑦  become  the 
dependent variables and the curvilinear coordinates 𝜉 , 𝜂 the independent variables.  By 
the usual methods of changing variables we obtain 
𝛼𝑥𝜉𝜉 − 2𝛽𝑥𝜉𝜂 + 𝛾𝑥𝜂𝜂 = 0,
𝛼𝑦𝜉𝜉 − 2𝛽𝑦𝜉𝜂 + 𝛾𝑦𝜂𝜂 = 0,
where 
𝛼 ≡ 𝑥𝜂
2 + 𝑦𝜂
2,    𝛽 ≡ 𝑥𝜉 𝑥𝜂 + 𝑦𝜉 𝑦𝜂, 𝛾 ≡ 𝑥𝜉
2.
2 + 𝑦𝜉
Equations (16.1.2) can be written in vector form: 
𝛼𝐫𝜉𝜉 − 2𝛽𝐫𝜉𝜂 + 𝛾𝐫𝜂𝜂 = 𝟎,
where 
𝐫 ≡ 𝑥𝐢 + 𝑦𝐣.
(20.1.2a)
(20.1.2b)
(20.1.3)
(20.1.4)
(20.1.5)
We  differentiate  Equations  (20.1.4)  and  solve  them  numerically  by  an  iterative 
method,  since  they  are  nonlinear.    In  (𝜉 , 𝜂)  space,  we  use  a  mesh  whose  curvilinear 
coordinates  are  straight  lines  which  take  on  integer values  corresponding  to  the  usual 
numbering  in  a  two-dimensional  mesh.    The  numerical  solution  then  gives  us  the 
location of the “equipotential” mesh lines. 
In  three  dimensions 𝑥,  𝑦,  𝑧,  we  add  a  third  curvilinear  coordinate 𝜁   and  a  third 
Laplace equation
LS-DYNA Theory Manual 
Simplified Arbitrary Lagrangian-Eulerian 
∇2𝜁 = 0.
(20.1.1c)
Inversion of the system of three equations (17.1.1) by change of variable is rather 
complicated.    It  is  easier,  as  well  as  more  illuminating,  to  use  the  methods  of  tensor 
analysis  pioneered  by Warsi [1982].    Let  the curvilinear  coordinates  be  represented  by 
𝜉 𝑖(𝑖 = 1,2,3).  For a scalar function 𝐴(𝑥, 𝑦, 𝑧),Warsi shows that the transformation of its 
Laplacian from rectangular Cartesian to curvilinear coordinates is given by  
∇2𝐴 = ∑ 𝑔𝑖𝑗𝐴𝜉 𝑖𝜉 𝑗 + ∑(∇2𝜉 𝑘)𝐴𝜉 𝑘
,
(20.1.6)
𝑖,𝑗=1
𝑘=1
where a variable subscript indicates differentiation with respect to that variable.  Since 
the  curvilinear  coordinates  are  each  assumed  to  satisfy  Laplace’s  equation,  the  second 
summation in Equation (20.1.6) vanishes and we have 
∇2𝐴 = ∑ 𝑔𝑖𝑗𝐴𝜉 𝑖𝜉 𝑗
.
𝑖,𝑗=1
(20.1.7)
If now we let 𝐴 = 𝑥, 𝑦, and 𝑧 successively, the left-hand side of (20.1.7) vanishes 
in each case and we get three equations which we can write in vector form 
∑ 𝑔𝑖𝑗𝐫𝜉 𝑖𝜉 𝑗 = 0
.
𝑖,𝑗=1
(20.1.8)
Equation  (20.1.8)  is  the  three-dimensional  generalization  of  Equations  (20.1.4), 
and it only remains to determine the components of the contravariant metric tensor 𝑔𝑖𝑗 
in three dimensions.  These are defined to be 
𝑔𝑖𝑗 ≡ 𝐚𝑖 ⋅ 𝐚𝑗,
(20.1.9)
where  the  contravariant  base  vectors  of  the  transformation  from  (𝑥, 𝑦, 𝑧)  to (𝜉 1, 𝜉 2, 𝜉 3) 
are given by 
𝐚𝑖 ≡ ∇𝜉 𝑖 =
𝐚𝑗 × 𝐚𝑘
√𝑔
,
(20.1.10)
(𝑖, 𝑗, 𝑘 cyclic).  Here the covariant base vectors, the coordinate derivatives, are given by 
𝐚𝑖 ≡ 𝐫𝜉 𝑖,
𝐫 ≡ 𝑥ı̂ + 𝑦ĵ + 𝑧𝐤̂ .
where  
Also,  
𝑔 ≡ det(𝑔𝑖𝑗) = [𝐚1 ⋅ (𝐚2 × 𝐚3)]2 = 𝐽2,
(20.1.11)
(20.1.12)
(20.1.13)
Simplified Arbitrary Lagrangian-Eulerian 
LS-DYNA Theory Manual 
where 𝑔𝑖𝑗 is the covariant metric tensor given by 
𝑔𝑖𝑗 ≡ 𝐚𝑖 ⋅ 𝐚𝑗,
(20.1.14)
and 𝐽 is the Jacobian of the transformation. 
Substituting (20.1.10) into (20.1.9), and using the vector identity  
(𝐚 × 𝐛) ⋅ (𝐜 × 𝐝) ≡ (𝐚 ⋅ 𝐜) ⋅ (𝐛 ⋅ 𝐝) − (𝐚 ⋅ 𝐝)(𝐛 ⋅ 𝐜),
(20.1.15)
we get 
𝑔𝑔𝑖𝑖 = 𝐚𝑗
2𝐚𝑘
2 − (𝐚𝑗 ⋅ 𝐚𝑘)
= 𝑔𝑗𝑗𝑔𝑘𝑘 − (𝑔𝑗𝑘)
,
𝑔𝑔𝑖𝑗 = (𝐚𝑖 ⋅ 𝐚𝑘)(𝐚𝑗 ⋅ 𝐚𝑘) − (𝐚𝑖 ⋅ 𝐚𝑗)𝐚𝑘
2 = 𝑔𝑖𝑘𝑔𝑗𝑘 − 𝑔𝑖𝑗𝑔𝑘𝑘.
(20.1.16)
(20.1.17)
Before substituting (20.1.11) into (17.1.13a, b), we return to our original notation:  
Then, using (20.1.11), we get 
𝜉 + 𝜉 1, 𝜂 + 𝜉 2, 𝜁 + 𝜉 3.
𝑔𝑔11 = 𝐫𝜂
2𝐫𝜁
2 − (𝐫𝜂 ⋅ 𝐫𝜁 )
𝑔𝑔22 = 𝐫𝜁
2𝐫𝜉
2 − (𝐫𝜁 ⋅ 𝐫𝜉 )
𝑔𝑔33 = 𝐫𝜉
2𝐫𝜂
2 − (𝐫𝜉 ⋅ 𝐫𝜂)
,
,
,
for the three diagonal components, and 
2,
𝑔𝑔12 = (𝐫𝜉 ⋅ 𝐫𝜁 )(𝐫𝜂 ⋅ 𝐫𝜁 ) − (𝐫𝜉 ⋅ 𝐫𝜂)𝐫𝜁
2,
𝑔𝑔23 = (𝐫𝜂 ⋅ 𝐫𝜉 )(𝐫𝜁 ⋅ 𝐫𝜉 ) − (𝐫𝜂 ⋅ 𝐫𝜁 )𝐫𝜉
2,
𝑔𝑔31 = (𝐫𝜁 ⋅ 𝐫𝜂)(𝐫𝜉 ⋅ 𝐫𝜂) − (𝐫𝜁 ⋅ 𝐫𝜉 )𝐫𝜂
(20.1.18)
(20.1.19)
(20.1.20)
(20.1.21)
(20.1.22)
(20.1.23)
(20.1.24)
for the three off-diagonal components of this symmetric tensor. 
When we express Equations (17.1.15) in terms of the Cartesian coordinates, some 
cancellation takes place and we can write them in the form 
𝑔𝑔11 = (𝑥𝜂𝑦𝜁 − 𝑥𝜁 𝑦𝜂)2 + (𝑥𝜂𝑧𝜁 − 𝑥𝜁 𝑧𝜂)2 + (𝑦𝜂𝑧𝜁 − 𝑦𝜁 𝑧𝜂)2, 
𝑔𝑔22 = (𝑥𝜁 𝑦𝜉 − 𝑥𝜉 𝑦𝜁 )2 + (𝑥𝜁 𝑧𝜉 − 𝑥𝜉 𝑧𝜁 )2 + (𝑦𝜁 𝑧𝜉 − 𝑦𝜉 𝑧𝜁 )2, 
𝑔𝑔33 = (𝑥𝜉 𝑦𝜂 − 𝑥𝜂𝑦𝜉 )2 + (𝑥𝜉 𝑧𝜂 − 𝑥𝜂𝑧𝜉 )2 + (𝑦𝜉 𝑧𝜂 − 𝑦𝜂𝑧𝜉 )2, 
(20.1.25)
(20.1.26)
(20.1.27)
guaranteeing  positivity  as  required  by  Equations  (20.1.9).    Writing  out  Equations 
(17.1.16) we get
LS-DYNA Theory Manual 
Simplified Arbitrary Lagrangian-Eulerian 
𝑔𝑔12 = (𝑥𝜉 𝑥𝜁 + 𝑦𝜉 𝑦𝜁 + 𝑧𝜉 𝑧𝜁 )(𝑥𝜂𝑥𝜁 + 𝑦𝜂𝑦𝜁 + 𝑧𝜂𝑧𝜁 )
−(𝑥𝜉 𝑥𝜂 + 𝑦𝜉 𝑦𝜂 + 𝑧𝜉 𝑧𝜂)(𝑥𝜁
2 + 𝑦𝜁
2 + 𝑧𝜁
2),
𝑔𝑔23 = (𝑥𝜂𝑥𝜉 + 𝑦𝜂𝑦𝜉 + 𝑧𝜂𝑧𝜉 )(𝑥𝜁 𝑥𝜉 + 𝑦𝜁 𝑦𝜉 + 𝑧𝜁 𝑧𝜉 )
−(𝑥𝜂𝑥𝜁 + 𝑦𝜂𝑦𝜁 + 𝑧𝜂𝑧𝜁 )(𝑥𝜉
2 + 𝑦𝜉
2 + 𝑧𝜉
2),
𝑔𝑔31 = (𝑥𝜁 𝑥𝜂 + 𝑦𝜁 𝑦𝜂 + 𝑧𝜁 𝑧𝜂)(𝑥𝜉 𝑥𝜂 + 𝑦𝜉 𝑦𝜂 + 𝑧𝜉 𝑧𝜂)
−(𝑥𝜁 𝑥𝜉 + 𝑦𝜁 𝑦𝜉 + 𝑧𝜁 𝑧𝜉 )(𝑥𝜂
2 + 𝑦𝜂
2 + 𝑧𝜂
2).
(20.1.28)
(20.1.29)
(20.1.30)
Hence, we finally write Equations (20.1.8) in the form 
𝑔(𝑔11𝐫𝜉𝜉 + 𝑔22𝐫𝜂𝜂 + 𝑔33𝐫𝜁𝜁 + 2𝑔12𝐫𝜉𝜂 + 2𝑔23𝐫𝜂𝜁 + 2𝑔31𝐫𝜁𝜉 ) = 0, 
(20.1.31)
where the 𝑔𝑔𝑖𝑗 are given by Equations (17.1.17) and (17.1.18).  Because Equations (20.1.8) 
are homogeneous, we can use 𝑔𝑔𝑖𝑗 in place of 𝑔𝑖𝑗 as long as 𝑔 is positive, as it must be for 
a  nonsingular  transformation.    We  can  test  for  positivity  at  each  mesh  point  by  using 
Equation (1.1.32): 
√𝑔 = 𝐽 =
𝑥𝜉
𝑥𝜂
𝑥𝜁
∣
∣∣
∣
𝑦𝜉
𝑦𝜂
𝑦𝜁
𝑧𝜉
∣
𝑧𝜂
∣∣
, 
𝑧𝜁 ∣
(20.1.32)
and requiring that 𝐽  >  0. 
To  check  that  these  equations  reproduce  the  two-dimensional  equations  when 
there  is  no  variation  in  one-dimension,  we  take  𝜁    as  the  invariant  direction,  thus 
reducing (17.1.19) to 
𝑔𝑔11𝐫𝜉𝜉 + 2𝑔𝑔12𝐫𝜉𝜂 + 𝑔𝑔22𝐫𝜂𝜂 = 0.
If we let 𝜁 = 𝑧, then the covariant base vectors become 
𝐚1 = 𝑥𝜉 𝐢 + 𝑦𝜉 𝐣,
𝐚2 = 𝑥𝜂𝐢 + 𝑦𝜂𝐣,
𝐚3 = 𝐤.
From (17.1.22), using (17.1.13), we get 
𝑔𝑔11 = 𝑥𝜂
2,
2 + 𝑦𝜂
𝑔𝑔22 = 𝑥𝜉
2,
2 + 𝑦𝜉
𝑔𝑔12 = −(𝑥𝜉 𝑥𝜂 + 𝑦𝜉 𝑦𝜂).
(20.1.33)
(20.1.34)
(20.1.35)
(20.1.36)
(20.1.37)
(20.1.38)
(20.1.39)
Substituting  (17.1.23)  into  (20.1.33)  yields  the  two-dimensional  equipotential  zoning 
Equations (17.1.2).
Simplified Arbitrary Lagrangian-Eulerian 
LS-DYNA Theory Manual 
Before differencing Equations (17.1.19) we simplify the notation and write them 
in the form 
where 
𝛼1𝐫𝜉𝜉 + 𝛼2𝐫𝜂𝜂 + 𝛼3𝐫𝜁𝜁 + 2𝛽1𝐫𝜉𝜂 + 2𝛽2𝐫𝜂𝜁 + 2𝛽3𝐫𝜁𝜉 = 0,
(20.1.40)
𝛼1 = (𝑥𝜂𝑦𝜁 − 𝑥𝜁 𝑦𝜂)2 + (𝑥𝜂𝑧𝜁 − 𝑥𝜁 𝑧𝜂)2 + (𝑦𝜂𝑧𝜁 − 𝑦𝜁 𝑧𝜂)2,
𝛼2 = (𝑥𝜁 𝑦𝜉 − 𝑥𝜉 𝑦𝜁 )2 + (𝑥𝜁 𝑧𝜉 − 𝑥𝜉 𝑧𝜁 )2 + (𝑦𝜁 𝑧𝜉 − 𝑦𝜉 𝑧𝜁 )2,
𝛼3 = (𝑥𝜉 𝑦𝜂 − 𝑥𝜂𝑦𝜉 )2 + (𝑥𝜉 𝑧𝜂 − 𝑥𝜂𝑧𝜉 )2 + (𝑦𝜉 𝑧𝜂 − 𝑦𝜂𝑧𝜉 )2.
𝛽1 = (𝑥𝜉 𝑥𝜁 + 𝑦𝜉 𝑦𝜁 + 𝑧𝜉 𝑧𝜁 )(𝑥𝜂𝑥𝜁 + 𝑦𝜂𝑦𝜁 + 𝑧𝜂𝑧𝜁 )
−(𝑥𝜉 𝑥𝜂 + 𝑦𝜉 𝑦𝜂 + 𝑧𝜉 𝑧𝜂)(𝑥𝜁
2 + 𝑦𝜁
2 + 𝑧𝜁
2),
𝛽2 = (𝑥𝜂𝑥𝜉 + 𝑦𝜂𝑦𝜉 + 𝑧𝜂𝑧𝜉 )(𝑥𝜉 𝑥𝜁 + 𝑦𝜉 𝑦𝜁 + 𝑧𝜉 𝑧𝜁 )
−(𝑥𝜁 𝑥𝜂 + 𝑦𝜁 𝑦𝜂 + 𝑧𝜁 𝑧𝜂)(𝑥𝜉
2 + 𝑦𝜉
2 + 𝑧𝜉
2),
𝛽3 = (𝑥𝜂𝑥𝜁 + 𝑦𝜂𝑦𝜁 + 𝑧𝜂𝑧𝜁 )(𝑥𝜉 𝑥𝜂 + 𝑦𝜉 𝑦𝜂 + 𝑧𝜉 𝑧𝜂)
−(𝑥𝜉 𝑥𝜂 + 𝑦𝜉 𝑦𝜂 + 𝑧𝜉 𝑧𝜂)(𝑥𝜂
2 + 𝑦𝜂
2 + 𝑧𝜂
2),
(20.1.41)
(20.1.42)
(20.1.43)
(20.1.44)
(20.1.45)
(20.1.46)
We  difference  Equations  (20.1.40)  in  a  cube  in  the  rectangular  𝜉  𝜂 𝜁   space  with 
unit  spacing  between  the  coordinate  surfaces,  using  subscript  𝑖  to  represent  the  𝜉  
direction, 𝑗 the 𝜂 direction, and 𝑘 the 𝜁  direction, as shown in Figure 20.1.
LS-DYNA Theory Manual 
Simplified Arbitrary Lagrangian-Eulerian 
Figure 20.1.  Example Caption 
Using  central  differencing,  we  obtain  the  following  finite  difference  approxima-
tions for the coordinate derivatives:  
𝐫𝜉 = (𝐫𝑖+1 − 𝐫𝑖−1) 2,⁄
𝐫𝜂 = (𝐫𝑗+1 − 𝐫𝑗−1) 2⁄ ,
𝐫𝜁 = (𝐫𝑘+1 − 𝐫𝑘−1) 2⁄ ,
𝐫𝜉𝜉 = (𝐫𝑖+1 − 2𝐫 + 𝐫𝑖−1),
𝐫𝜂𝜂 = (𝐫𝑗+1 − 2𝐫 + 𝐫𝑗−1),
𝐫𝜁𝜁 = (𝐫𝑘+1 − 2𝐫 + 𝐫𝑘−1),
𝐫𝜉𝜂 =
[(𝐫𝑖+1,𝑗+1 + 𝐫𝑖−1,𝑗−1) − (𝐫𝑖+1,𝑗−1 + 𝐫𝑖−1,𝑗+1)],
𝐫𝜂𝜁 =
𝐫𝜁𝜉 =
[(𝐫𝑗+1,𝑘+1 + 𝐫𝑗−1,𝑘−1) − (𝐫𝑗+1,𝑘−1 + 𝐫𝑗−1,𝑘+1)],
[(𝐫𝐼+1,𝑘+1 + 𝐫𝐼−1,𝑘−1) − (𝐫𝐼+1,𝑘−1 + 𝐫𝐼−1,𝑘+1)],
(20.1.47)
(20.1.48)
(20.1.49)
(20.1.50)
(20.1.51)
(20.1.52)
(20.1.53)
(20.1.54)
(20.1.55)
where for brevity we have omitted subscripts 𝑖, 𝑗, or 𝑘 (e.g., 𝑘 + 1 stands for 𝑖, 𝑗, 𝑘  +  1).  
Note that these difference expressions use only coordinate planes that pass through the 
central point, and therefore do not include the eight corners of the cube.
Simplified Arbitrary Lagrangian-Eulerian 
LS-DYNA Theory Manual 
Substituting Equations (17.1.26) into (17.1.24,17.1.25) and collecting terms, we get 
18
∑
𝑚=1
𝜔𝑚(𝐫𝑚 − 𝐫) = 0,
(20.1.56)
where  the  sum  is  over  the  18  nearest  (in  the  transform  space)  neighbors  of  the  given 
point.  The coefficients 𝜔𝑚 are given in Table 17.1. 
Equations (20.1.56) can be written 
𝐫𝑚 =
∑ 𝜔𝑚𝐫𝑚
∑ ω𝑚𝑚
,
(20.1.57)
expressing  the  position  of  the  central  point  as  a  weighted  mean  of  its  18  nearest 
neighbors.  The denominator of (20.1.57) is equal to 2(𝛼1 + 𝛼2 + 𝛼3) which is guaranteed 
to  be  positive  by  (17.1.25).    This  vector  equation  is  equivalent  to  the  three  scalar 
equations 
(20.1.58)
(20.1.59)
𝑥 =
∑ 𝜔𝑚x𝑚
∑ ω𝑚𝑚
,
𝑦 =
∑ 𝜔𝑚y𝑚
∑ 𝜔𝑚𝑚
,
Index 
𝑖 + 1
𝑖– 1
𝑗 + 1
𝑗– 1
𝑘 + 1
𝑘– 1
𝑖 + 1, 𝑗 + 1
𝑖– 1, 𝑗– 1
𝑖 + 1, 𝑗– 1
𝑖– 1, 𝑗 + 1
𝑗 + 1, 𝑘 + 1
𝑗– 1, 𝑘– 1
𝑗 + 1, 𝑘– 1
𝑗– 1, 𝑘 + 1
𝑖 + 1, 𝑘 + 1
𝑖– 1, 𝑘– 1
𝑖 + 1, 𝑘– 1
𝑖– 1, 𝑘 + 1
 m 
  1 
  2 
  3 
  4 
  5 
  6 
  7 
  8 
  9 
10 
11 
12 
13 
14 
15 
16 
17 
18 
𝜔𝑚
𝛼1
𝛼1
𝛼2
𝛼2
𝛼3
𝛼3
𝛽1/2 
𝛽1/2 
−𝛽1/2 
−𝛽1/2 
𝛽2/2 
𝛽2/2 
−𝛽2/2 
−𝛽2/2 
𝛽3/2 
𝛽3/2 
−𝛽3/2 
−𝛽3/2
LS-DYNA Theory Manual 
Simplified Arbitrary Lagrangian-Eulerian 
Table 17.1.  3D Zoning Weight Coefficients 
𝑧 =
∑ 𝜔𝑚𝑧𝑚
∑ 𝜔𝑚𝑚
.
(20.1.60)
the same weights 𝜔𝑚 appearing in each equation. 
These  equations  are  nonlinear,  since  the  coefficients  are  functions  of  the 
coordinates.    Therefore  we  solve  them  by  an  iterative  scheme,  such  as  SOR.    When 
applied to Equation (20.1.58), for example, this gives for the (n+1)st iteration 
𝑥𝑛+1 = (1 − f)𝑥𝑛 + f (
∑ 𝜔𝑚𝑥𝑚
∑ 𝜔𝑚𝑚
),
(20.1.61)
where the over relaxation factor 𝑓  must satisfy 0 < 𝑓 < 2.  In (20.1.61) the values of 𝑥𝑚 at 
the  neighboring  points  are  the  latest  available  values.    The  coefficients  𝜔𝑚  are 
recalculated before each iteration using Table 17.1 and Equations (17.1.25).   
To  smooth  one  interior  point  in  a  three-dimensional  mesh,  let  the  point  to  be 
smoothed  be  the  interior  point  of  Figure  17.1,  assuming  that  its  neighborhood  has  the 
logical structure shown.  Even though Equations (17.1.29) are nonlinear, the 𝜔𝑚 do not 
involve  the  coordinates  of  the  central  point,  since  the  α’s  and β’s  do  not.    Hence  we 
simply  solve  Equations  (17.1.29)  for  the  new  coordinates  (𝑥, 𝑦, 𝑧),  holding  the  18 
neighboring points fixed, without needing to iterate. 
If  we  wish  to  smooth  a  group  of  interior  points,  we  solve  iteratively  for  the 
coordinates using equations of the form (20.1.61). 
20.1.2  Simple Averaging 
The  coordinates  of  a  node  is  the  simple  average  of  the  coordinates  of  its 
surrounding nodes. 
𝑛+1 =
𝑥SA
𝑚tot
𝑚tot ∑ 𝑥𝑚
𝑚=1
.
(20.1.62)
20.1.3  Kikuchi’s Algorithm 
 Kikuchi  proposed  an  algorithm  that  uses  a  volume-weighted  average  of  the 
coordinates  of  the  centroids  of  the  elements  surrounding  a  node.    Variables  that  are 
subscripted  with  Greek  letters  refer  to  element  variables,  and  subscripts  with  capital 
letters refer to the local node numbering within an element. 
n =
𝑥α
∑ 𝑥𝐴
,
(20.1.63)
Simplified Arbitrary Lagrangian-Eulerian 
LS-DYNA Theory Manual 
𝑛+1 =
𝑥𝐾
αtot
∑ 𝑉a𝑥α
α=1
αtot
∑ Va
α=1
. 
(20.1.64)
20.1.4  Surface Smoothing 
The  surfaces  are  smoothed  by  extending  the  two-dimensional  equipotential 
stencils to three dimensions.  Notice that the form of Equation (20.1.2a) and (20.1.2b) for 
the 𝑥 and 𝑦 directions are identical.  The third dimension, 𝑧, takes the same form.  When 
Equation  (16.1.2)  is  applied  to  all  three  dimensions,  it  tends  to  flatten  out  the  surface 
and  alter  the  total  volume.    To  conserve  the  volume  and  retain  the  curvature  of  the 
surface,  the  point  given  by  the  relaxation  stencil  is  projected  on  to  the  tangent  plane 
defined by the normal at the node. 
20.1.5  Combining Smoothing Algorithms 
The  user  has  the  option  of  using  a  weighted  average  of  all  three  algorithms  to 
generate  a  composite  algorithm,  where  the  subscripts  E,  SA,  and  K  refer  to  the 
equipotential,  simple  averaging,  and  Kikuchi’s  smoothing  algorithm  respectively,  and 
ww is the weighting factor.  
𝑥𝑛+1 = 𝑤E𝑥E
𝑛+1 + 𝑤SA𝑥SA
𝑛+1 + 𝑤K𝑥K
𝑛+1.
(20.1.65)
20.2  Advection Algorithms 
LS-DYNA  follows  the  SALE3D  strategy  for  calculating  the  transport  of  the 
element-centered  variables  (i.e.,  density,  internal  energy,  the  stress  tensor  and  the 
history variables).  The van Leer MUSCL scheme [van Leer 1977] is used instead of the 
donor  cell  algorithm  to  calculate  the  values  of  the  solution  variables  in  the  transport 
fluxes to achieve second order accurate monotonic results.  To calculate the momentum 
transport, two algorithms have been implemented.  The less expensive of the two is the 
one  that  is  implemented  in  SALE3D,  but  it  has  known  dispersion  problems  and  may 
violate  monotonocity  (i.e.,  introduce  spurious  oscillations)  [Benson  1992].    As  an 
alternative, a significantly more expensive method [Benson 1992], which can be shown 
analytically to not have either problem on a regular mesh, has also been implemented. 
In this section the donor cell and van Leer MUSCL scheme are discussed.  Both 
methods  are  one-dimensional  and  their  extensions  to  multidimensional  problems  are 
discussed later. 
20.2.1  Advection Methods in One Dimension 
In this section the donor cell and van Leer MUSCL scheme are discussed.  Both 
methods  are  one-dimensional  and  their  extensions  to  multidimensional  problems  are 
discussed later.
LS-DYNA Theory Manual 
Simplified Arbitrary Lagrangian-Eulerian 
The  remap  step  maps  the  solution  from  a  distorted  Lagrangian  mesh  on  to  the 
new  mesh.    The  underlying  assumptions  of  the  remap  step  are  1)  the  topology  of  the 
mesh is fixed (a complete rezone does not have this limitation), and 2) the mesh motion 
during a step is less than the characteristic lengths of the surrounding elements.  Within 
the  fluids  community,  the  second  condition  is  simply  stated  as  saying  the  Courant 
number, 𝐶, is less than one. 
𝐶 =
𝑢Δ𝑡
Δ𝑥
=
≤ 1,
(20.2.66)
Since  the  mesh  motion  does  not  occur  over  any  physical  time  scale,  Δt  is 
arbitrary, and uΔt is the transport volume, 𝑓 , between adjacent elements.  The transport 
volume calculation is purely geometrical for ALE formulations and it is not associated 
with any of the physics of the problem. 
The algorithms for performing the remap step are taken from the computational 
fluids  dynamics  community,  and  they  are  referred  to  as  “advection”  algorithms  after 
the  first  order,  scalar  conservation  equation  that  is  frequently  used  as  a  model 
hyperbolic problem.  
∂φ
∂t
+ a(𝑥)
∂φ
∂𝑥
= 0.
(20.2.67)
A  good  advection  algorithm  for  the remap step  is  accurate,  stable,  conservative 
and monotonic.  Although many of the solution variables, such as the stress and plastic 
strain, are not governed by conservation equations like momentum and energy, it is still 
highly desirable that the volume integral of all the solution variables remain unchanged 
by the remap step.  Monotonicity requires that the range of the solution variables does 
not  increase  during  the  remap.    This  is  particularly  important  with  mass  and  energy, 
where negative values would lead to physically unrealistic solutions. 
Much  of  the  research  on  advection  algorithms  has  focused  on  developing 
monotonic  algorithms  with  an  accuracy  that  is  at  least  second  order.    Not  all  recent 
algorithms  are  monotonic.    For  example,  within  the  finite  element  community,  the 
streamline  upwind  Petrov-Galerkin  (SUPG)  method  developed  by  Hughes  and 
coworkers  [Brooks  and  Hughes  1982]  is  not  monotonic.    Johnson  et  al.,  [1984]  have 
demonstrated  that  the  oscillations  in  the  SUPG  solution  are  localized,  and  its 
generalization  to  systems  of  conservation  equations  works  very  well  for  the  Euler 
equations. 
  Mizukami  and  Hughes  [1985]  later  developed  a  monotonic  SUPG 
formulation.    The  essentially  non-oscillatory  (ENO)  [Harten  1989]  finite  difference 
algorithms  are  also  not  strictly  monotonic,  and  work  well  for  the  Euler  equations,  but 
their  application  to  hydrodynamics  problems  has  resulted  in  negative  densities 
[McGlaun 1990].  Virtually all the higher order methods that are commonly used were 
originally developed for solving the Euler equations, usually as higher order extensions
Simplified Arbitrary Lagrangian-Eulerian 
LS-DYNA Theory Manual 
to  Godunov’s  method.    Since  the  operator  split  approach  is  the  dominant  one  in 
Eulerian hydrocodes, these methods are implemented only to solve the scalar advection 
equation. 
The Donor Cell Algorithm.  Aside from its first order accuracy, it is everything a good 
𝜑  is 
advection  algorithm  should  be:  stable,  monotonic,  and  simple.    The  value  of  𝑓𝑗
dependent on the sign of a at node 𝑗, which defines the upstream direction.  
𝑛+1 = φ𝑗+1
φ𝑗+1
2⁄
2⁄
+
Δ𝑡
Δ𝑥
(𝑓𝑗
𝜑 − 𝑓𝑗+1
𝜑 ),
𝜑 =
𝑓𝑗
𝑎𝑗
(φ𝑗−1
2⁄
+ φ𝑗+1
2⁄
) +
|𝑎𝑗|
(φ𝑗−1
2⁄
− φ𝑗+1
2⁄
).
(20.2.68)
(20.2.69)
The  donor  cell  algorithm  is  a  first  order  Godunov  method  applied  to  the 
advection equation.  The initial values of 𝜙 to the left and the right of node 𝑗 are φ𝑗−1
2⁄
and φ𝑗+1
2⁄
, and the velocity of the contact discontinuity at node 𝑗 is 𝑎𝑗.  
The Van Leer MUSCL Algorithm. Van Leer [1977] introduced a family of higher order 
Godunov  methods  by  improving  the  estimates  of  the  initial  values  of  left  and  right 
states for the Riemann problem at the nodes.  The particular advection algorithm that is 
presented  in  this  section  is  referred  to  as  the  MUSCL  (monotone  upwind  schemes  for 
conservation laws) algorithm for brevity, although MUSCL really refers to the family of 
algorithms that can be applied to systems of equations. 
The  donor  cell  algorithm  assumes  that  the  distribution  of  𝜙  is  constant  over  an 
element.    Van  Leer  replaces  the  piecewise  constant  distribution  with  a  higher  order 
interpolation  function,  φ𝑗+1
(𝑥)  that  is  subject  to  an  element  level  conservation 
2⁄
constraint.    The  value  of  𝜙  at  the  element  centroid  is  regarded  in  this  context  as  the 
average value of 𝜙 over the element instead of the spatial value at 𝑥𝑗+1
2⁄ . 
φ𝑗+1
2⁄
𝑥𝑗+1
= ∫
𝑥𝑗
φ𝑗+1
2⁄
(𝑥)d𝑥,
(20.2.70)
min , φ𝑗+1
To  determine  the  range  of  𝜙,  [φ𝑗+1
2⁄
2⁄
max ],  for  imposing  the  monotonicity 
constraint,  the  maximum  and  minimum  values  of  φ𝑗−1
2⁄
Monotonicity  can  be  imposed  in  either  of  two  ways.    The  first  is  to  require  that  the 
(𝑥)  fall  within  the  range  determined  by  the 
maximum  and  minimum  values  of  φ𝑗+1
2⁄
three elements.  The second is to restrict the average value of 𝜙 in the transport volumes 
associated  with  element   𝑗 + 1/2.    While  the  difference  may  appear  subtle,  the  actual 
difference between the two definitions is quite significant even at relatively low Courant 
numbers.  The second definition allows the magnitude of the 𝜙 transported to adjacent 
,  and  φ𝑗+3
2⁄
  are  used.  
,  φ𝑗+1
2⁄
LS-DYNA Theory Manual 
Simplified Arbitrary Lagrangian-Eulerian 
elements to be larger than the first definition.  As a consequence, the second definition is 
better  able  to  transport  solutions  with  large  discontinuities.    The  magnitude  of  𝜙  an 
algorithm is able to transport before its monotonicity algorithm restricts 𝜙 is a measure 
of the algorithm’s “compressiveness.” 
The  first  step  up  from  a  piecewise  constant  function  is  a  piecewise  linear 
function,  where 𝑥 is now the volume coordinate.  The volume  coordinate of a point is 
simply  the  volume  swept  along  the  path  between  the  element  centroid  and  the  point.  
Conservation  is  guaranteed  by  expanding  the  linear  function  about  the  element 
centroid. 
φ𝑗+1
2⁄
(𝑥) = 𝑆𝑗+1
2⁄
(𝑥 − 𝑥𝑗+1
2⁄
) + φj+1
2⁄
.
(20.2.71)
Letting  𝑠𝑗+1
2⁄
  be  a  second  order  approximation  of  the  slope,  the  monotonicity 
limited value of the slope, 𝑠𝑗+1
2⁄
by assuming the maximum permissible values at the element boundaries. 
, according to the first limiting approach, is determined 
𝑆𝑗+1
2⁄
=
(sgn(sL) + sgn(sR)) × min (∣sL∣, ∣s𝑗+1
2⁄
∣ , ∣sR∣), 
𝑠L =
𝑠R =
− φ𝑗−1
2⁄
φ𝑗+1
2⁄
Δ𝑥𝑗+1
2⁄
− φ𝑗+1
2⁄
φ𝑗+3
2⁄
Δ𝑥𝑗+1
2⁄
, 
. 
(20.2.72)
(20.2.73)
(20.2.74)
The  second  limiter  is  similar  to  the  first,  but  it  assumes  that  the  maximum 
permissible values occur at the centroid of the transport volumes.  Note that as stated in 
Equation  (17.2.6),  this  limiter  still  limits  the  slope  at  the  element  boundary  even  if  the 
element  is  the  downstream  element  at  that  boundary.    A  more  compressive  limiter 
would not limit the slope based on the values of 𝜙 at the downstream boundaries.  For 
example, if 𝑎𝑗 is negative, only 𝑆𝑅 would limit the value of 𝑆𝑛 in Equation (17.2.6).  If the 
element  is  the  downstream  element  at  both  boundaries,  then  the  slope  in  the  element 
has no effect on the solution. 
Δ𝑥𝑗+1
max(0, 𝑎𝑗Δ𝑡)
𝑠L =
𝑠R =
− φ𝑗−1
2⁄
− φ𝑗+1
2⁄
φ𝑗+1
2⁄
2⁄ − 1
φ𝑗+3
2⁄
2⁄ + 1
𝑥𝑗+1
min(0, 𝑎𝑗+1Δ𝑡)
. 
. 
(20.2.75)
(20.2.76)
Simplified Arbitrary Lagrangian-Eulerian 
LS-DYNA Theory Manual 
The flux at node 𝑗 is evaluated using the upstream approximation of 𝜙. 
φ =
𝑓𝑗
𝑎𝑗
(φ𝑗
− + φ𝑗
+) +
|𝑎𝑗|
(φ𝑗
− − φ𝑗
+),
+ = S𝑗+1
φ𝑗
2⁄
(𝑥C − 𝑥𝑗+1
2⁄
) + φ𝑗+1
2⁄
− = S𝑗−1
φ𝑗
2⁄
(𝑥C − 𝑥𝑗−1
2⁄
) + φ𝑗−1
2⁄
,
,
𝑥C = 𝑥𝑗
𝑛 +
𝑎𝑗Δ𝑡.
(20.2.77)
(20.2.78)
(20.2.79)
(20.2.80)
The  method  for  obtaining  the  higher  order  approximation  of  the  slope  is  not 
unique.  Perhaps the simplest approach is to fit a parabola through the centroids of the 
three  adjacent  elements  and  evaluate  its  slope  at  𝑥𝑗+1
.    When  the  value  of  𝜙  at  the 
2⁄
element centroids is assumed to be equal to the element average this algorithm defines 
a projection.  
(𝜑𝑗+3
2⁄
𝑠𝑗+1
2⁄
=
− φ𝑗+1
2⁄
) Δ𝑥𝑗
2 + (φ𝑗+1
2⁄
Δ𝑥𝑗Δ𝑥𝑗+1(Δ𝑥𝑗 + Δ𝑥𝑗+1)
− φ𝑗−1
2⁄
Δ𝑥𝑗 = 𝑥𝑗+1
2⁄
− 𝑥𝑗−1
2⁄
.
) Δ𝑥𝑗+1
,
(20.2.81)
(20.2.82)
20.2.2  Advection Methods in Three Dimensions 
For  programs  that  use  a  logically  regular  mesh,  one-dimensional  advection 
methods  are  extended  to  two  and  three  dimensions  by  using  a  sequence  of  one-
dimensional  sweeps  along  the  logically  orthogonal  mesh  lines.    This  strategy  is  not 
possible  for  unstructured  meshes  because  they  don’t  have  uniquely  defined  sweep 
directions  through  the  mesh.    CAVEAT  [Addessio,  et al.,  1986]  uses  one-dimensional 
sweeps in the spatial coordinate system, but their approach is expensive relative to the 
other  algorithms  and  it  does  not  always  maintain  spherical  symmetry,  which  is  an 
important consideration in underwater explosion calculations. 
The advection in LS-DYNA is performed isotropically.  The fluxes through each 
face  of  element  A  are  calculated  simultaneously,  but  the  values  of  𝜙  in  the  transport 
volumes  are  calculated  using  the  one-dimensional  expressions  developed  in  the 
previous sections.  
𝑛+1 =
φA
𝑛+1
VA
⎜⎛VA
⎝
𝑛 φA
𝑛 + ∑ f𝑗
⎟⎞.
𝑗=1 ⎠
(20.2.83)
LS-DYNA Theory Manual 
Simplified Arbitrary Lagrangian-Eulerian 
The disadvantage of isotropic advection is that there is no coupling between an 
element  and  the  elements  that  are  joined  to  it  only  at  its  corners  and  edges  (i.e., 
elements that don’t share faces).  The lack of coupling introduces a second order error 
that is significant only when the transport is along the mesh diagonals. 
The one-dimensional MUSCL scheme, which requires elements on either side of 
the  element  whose  transport  is  being  calculated,  cannot  be  used  on  the  boundary 
elements in the direction normal to the boundary.  Therefore, in the boundary elements, 
the donor cell algorithm is used to calculate the transport in the direction that is normal 
to the boundary, while the MUSCL scheme is used in the two tangential directions. 
It  is  implicitly  assumed  by  the  transport  calculations  that  the  solution  variables 
are defined per unit current volume.  In LS-DYNA, some variables, such as the internal 
energy, are stored in terms of the initial volume of the element.  These variables must be 
rescaled before transport, then the initial volume of the element is advected between the 
elements,  and  then  the  variables  are  rescaled  using  the  new  “initial”  volumes.  
Hyperelastic materials are not currently advected in LS-DYNA because they require the 
deformation gradient, which is calculated from the initial geometry of the mesh.  If the 
deformation gradient is integrated by using the midpoint rule, and it is advected with 
the  other  solution  variables,  then  hyperelastic  materials  can  be  advected  without  any 
difficulties. 
F𝑛+1 = (I −
Δ𝑡
2L𝑛+1
2⁄
)−1 (I +
Δ𝑡
2L𝑛+1
2⁄
) F𝑛.
(20.2.84)
Advection  of  the  Nodal  Velocities.    Except  for  the  Godunov  schemes,  the  velocity  is 
centered  at  the  nodes  or  the  edges  while  the  remaining  variables  are  centered  in  the 
elements.    Momentum  is  advected  instead  of  the  velocity  in  most  codes  to  guarantee 
that  momentum  is  conserved.    The  element-centered  advection  algorithms  must  be 
modified to advect the node-centered momentum.  Similar difficulties are encountered 
when node-centered algorithms, such as the SUPG method [Brooks and Hughes 1982], 
are applied to element-centered quantities [Liu, Chang, and Belytschko, to be published].  
There  are  two  approaches:  1)  construct  a  new  mesh  such  that  the  nodes  become  the 
element  centroids  of  the  new  mesh  and  apply  the  element-centered  advection 
algorithms,  and  2)  construct  an  auxiliary  set  of  element-centered  variables  from  the 
momentum,  advect  them,  and  then  reconstruct  the  new  velocities  from  the  auxiliary 
variables.    Both  approaches  can  be  made  to  work  well,  but  their  efficiency  is  heavily 
dependent on the architecture of the codes.  The algorithms are presented in detail for 
one  dimension  first  for  clarity.    Their  extensions  to  three  dimensions,  which  are 
presented  later,  are  straightforward  even  if  the  equations  do  become  lengthy.    A 
detailed  discussion  of  the  algorithms  in  two  dimensions  is  presented  in  Reference 
[Benson 1992].
Simplified Arbitrary Lagrangian-Eulerian 
LS-DYNA Theory Manual 
Notation.  Finite difference notation is used in this section so that the relative locations 
of  the  nodes  and  fluxes  are  clear.    The  algorithms  are  readily  applied,  however,  to 
unstructured meshes.  To avoid limiting the discussion to a particular element-centered 
advection algorithm, the transport volume through node 𝑖 is 𝑓 , the transported mass is 
𝑓 ̃
𝑖,  and  the  flux  of  𝜙  is  𝜙𝑖𝑓𝑖.    Most  of  the  element-centered  flux-limited  advection 
algorithms  calculate  the  flux  of  𝜙  directly,  but  the  mean  value  of  𝜙  in  the  transport 
volumes is calculated by dividing the 𝜙i𝑓i, by the transport volume.  A superscript “-” 
or “+” denotes the value of a variable before or after the advection.  Using this notation, 
the  advection  of  𝜙  in  one  dimension  is  represented  by  Equation  (17.2.12),  where  the 
volume is V. 
+
φ𝑗+1
2⁄
=
− V𝑗+1
(φ𝑗+1
2⁄
2⁄
−
+ φ𝑖𝑓𝑖 − φ𝑖+1𝑓𝑖+1)
,
V+
+
V𝑗+1
2⁄
−
= V𝑗+1
2⁄
+ 𝑓𝑖 − 𝑓𝑖+1.
(20.2.85)
(20.2.86)
The Staggered Mesh Algorithm.  YAQUI [Amsden and Hirt 1973] was the first code to 
construct  a  new  mesh  that  is  staggered  with  respect  to  original  mesh  for  momentum 
advection.  The new mesh is defined so that the original nodes become the centroids of 
the  new  elements.    The  element-centered  advection  algorithms  are  applied  to the  new 
mesh  to  advect  the  momentum.    In  theory,  the  momentum  can  be  advected  with  the 
transport volumes or the velocity can be advected with the mass. 
(M𝑗
−v𝑗
− + v𝑗−1
+ =
v𝑗
2⁄ − v𝑗+1
2⁄ 𝑓 ̃
𝑗+1
2⁄ )
,
(M𝑗
−v𝑗
− + {ρv}𝑗−1
+ =
v𝑗
2⁄ − {ρv}𝑗+1
2⁄ 𝑓𝑗−1
2⁄ )
,
2⁄ 𝑓 ̃
𝑗−1
+
M𝑗
2⁄ 𝑓𝑗−1
+
M𝑗
M𝑗
+ = M𝑗
− + 𝑓 ̃
𝑗−1
2⁄ − 𝑓 ̃
𝑗+1
2⁄ .
(20.2.87)
(20.2.88)
(20.2.89)
A  consistency  condition,  first  defined  by  DeBar  [1974],  imposes  a  constraint  on 
the formulation of the staggered mesh algorithm:  if a body has a uniform velocity and a 
spatially varying density before the advection, then the velocity should be uniform and 
unchanged after the advection.  The new mass of a node can be expressed in terms of 
the quantities used to advect the element-centered mass. 
+ =
M𝑗
+
(M𝑗−1
2⁄
+
+ M𝑗+1
2⁄
),
+ =
M𝑗
−
(M𝑗−1
2⁄
−
+ 𝜌𝑗−1𝑓𝑗−1 − 𝜌𝑗𝑓𝑗 + M𝑗+1
2⁄
+ 𝜌𝑗𝑓𝑗 − 𝜌𝑗+1𝑓𝑗+1), 
(20.2.90)
(20.2.91)
LS-DYNA Theory Manual 
Simplified Arbitrary Lagrangian-Eulerian 
M𝑗
+ = M𝑗
− +
[(𝜌𝑗−1𝑓𝑗−1 − 𝜌𝑗𝑓𝑗) + (𝜌𝑗𝑓𝑗 − 𝜌𝑗+1𝑓𝑗+1)].
(20.2.92)
The  staggered  mass  fluxes  and  transport  volumes  are  defined  by  equating  Equation 
(20.2.90) and Equation (17.2.15). 
𝜌𝑗+1
2⁄ 𝑓𝑗+1
2⁄ = 𝑓 ̃
𝑗+1
2⁄ =
(𝜌𝑗𝑓𝑗 + 𝜌𝑗+1𝑓𝑗+1).
(20.2.93)
2⁄   is  generally  a  nonlinear  function  of  the  volume  𝑓𝑗+1
2⁄ ,  hence 
The  density  𝜌𝑗+1
calculating  𝑓𝑗+1
2⁄   from  Equation  (20.2.93)  requires  the  solution  of  a  nonlinear  equation 
for each transport volume.  In contrast, the mass flux is explicitly defined by Equation 
(20.2.93).    Most  codes,  including  KRAKEN  [Debar  1974],  CSQ  [Thompson  1975],  CTH 
[McGlaun  1989],  and  DYNA2D  [Hallquist  1980],  use  mass  fluxes  with  the  staggered 
mesh algorithm because of their simplicity. 
The  dispersion  characteristics  of  this  algorithm  are  identical  to  the  underlying 
element-centered algorithm by construction.  This is not true, however, for some of the 
element-centered  momentum  advection  algorithms.    There  are  some  difficulties  in 
implementing  the  staggered  mesh  method  in  multi-dimensions.    First,  the  number  of 
edges  defining  a  staggered  element  equals  the  number  of  elements  surrounding  the 
corresponding node.  On an unstructured mesh, the arbitrary connectivity results in an 
arbitrary  number  of  edges  for  each  staggered  element.    Most  of  the  higher  order 
accurate  advection  algorithms  assume  a  logically  regular  mesh  of  quadrilateral 
elements,  making  it  difficult  to  use  them  with  the  staggered  mesh.    Vectorization  also 
becomes difficult because of the random number of edges that each staggered element 
might  have.    In  the  ALE  calculations  of  DYNA2D,  only  the  nodes  that  have  a  locally 
logically  regular  mesh  surrounding  them  can  be  moved  in  order  to  avoid  these 
difficulties  [Benson  1992].    These  difficulties  do  not  occur  in  finite  difference  codes 
which  process  logically  regular  blocks  of  zones.    Another  criticism  is  the  staggered 
mesh  algorithm  tends  to  smear  out  shocks  because  not  all  the  advected  variables  are 
element-centered  [Margolin  1989].    This  is  the  primary  reason,  according  to  Margolin 
[1989],  that  the  element-centered  algorithm  was  adopted  in  SALE  [Amdsden,  Ruppel, 
and Hirt  1980]. 
The SALE Algorithm. SALE advects an element-centered momentum and redistributes 
its changes to the nodes [Amdsden, Ruppel, and Hirt 1980].  The mean element velocity, 
𝐯̅̅̅̅𝑗+1
2⁄ ,  and  nodal  momentum 
2⁄ ,  specific  momentum,  𝐩𝑗+1
are defined by Equation (17.2.17). 
2⁄ ,  element  momentum,  𝐏𝑗+1
𝐯̅̅̅̅𝑗+1
2⁄ =
(𝐯𝑗 + 𝐯𝑗+1),
𝐩𝑗+1
2⁄ = ρ𝑗+1
2⁄ 𝐯̅̅̅̅𝑗+1
2⁄ ,
𝐏j+1
2⁄ = M𝑗+1
2⁄ 𝐯̅̅̅̅𝑗+1
2⁄ .
(20.2.94)
(20.2.95)
(20.2.96)
Simplified Arbitrary Lagrangian-Eulerian 
LS-DYNA Theory Manual 
2⁄ , the change in the velocity at a 
Denoting the change in the element momentum Δ𝐏𝑗+1
node  is  calculated  by  distributing  half  the  momentum  change  from  the  two  adjacent 
elements. 
Δ𝐏𝑗−1
2⁄ = p𝑗−1𝑓𝑗−1 − p𝑗𝑓𝑗,
+ = P𝑗
P𝑗
− +
(Δ𝐏𝑗−1
2⁄ + Δ𝐏𝑗+1
2⁄ ),
+ =
𝐯𝑗
+
𝐏𝑗
+.
M𝑗
(20.2.97)
(20.2.98)
(20.2.99)
This  algorithm  can  also  be  implemented  by  advecting  the  mean  velocity,  𝐯̅̅̅̅𝑗+1
2⁄  
with the transported mass, and the transported momentum 𝐩𝑗𝑓𝑗 is changed to 𝐯̅̅̅̅𝑗𝑓 ̃
𝑗. 
The  consistency  condition  is  satisfied  regardless  of  whether  masses  or  volumes 
are used.  Note that the velocity is not updated from the updated values of the adjacent 
element momenta.  The reason for this is the original velocities are not recovered if 𝑓𝑖 =
0, which indicates that there is an inversion error associated with the algorithm.  
The HIS (Half Index Shift) Algorithm.  Benson [1992] developed this algorithm based 
on  his  analysis  of  other  element-centered  advection  algorithms.    It  is  designed  to 
overcome the dispersion errors of the SALE algorithm and to preserve the monotonicity 
of  the  velocity  field.    The  SALE  algorithm  is  a  special  case  of  a  general  class  of 
algorithms.  To sketch the idea behind the HIS algorithm, the discussion is restricted to 
the scalar advection equation.  Two variables, Ψ1,𝑗+1
2⁄  are defined in terms 
of a linear transformation of 𝜙𝑗 and 𝜙𝑗+1.  The linear transformation may be a function 
of the element 𝑗 + 1/2. 
2⁄  and Ψ2,𝑗+1
−
{⎧Ψ1,𝑗+1
2⁄
−
⎩{⎨
Ψ2,𝑗+1
2⁄
}⎫
⎭}⎬
= [a b
c d
] {
−
φ𝑗
− }. 
φ𝑗+1
This relation is readily inverted. 
{
+
φ𝑗
+ } =
φ𝑗+1
ad − bc
−b
[d
−c a
]
+
{⎧Ψ1,𝑗+1
2⁄
⎩{⎨
+
Ψ2,𝑗+1
2⁄
}⎫
⎭}⎬
. 
(20.2.100)
(20.2.101)
A  function  is  monotonic  over  an  interval  if  its  derivative  does  not  change  sign.  
The sum of two monotonic functions is monotonic, but their difference is not necessarily 
  are  monotonic  over  the  same 
monotonic.    As  a  consequence,  Ψ1,𝑗+1
2⁄
− if all the coefficients in the linear transformation have the same sign.  On 
intervals as φ𝑗
  are 
the  other  hand,  φ𝑗
+  is  not  necessarily  monotonic  even  if  Ψ1,𝑗+1
2⁄
  and  Ψ2,𝑗+1
2⁄
  and  Ψ2,𝑗+1
2⁄
+
+
−
−
LS-DYNA Theory Manual 
Simplified Arbitrary Lagrangian-Eulerian 
monotonic  because  of  the  appearance  of  the  negative  signs  in  the  inverse  matrix.  
Monotonicity  can  be  maintained  by  transforming  in  both  directions  provided  that  the 
transformation  matrix  is  diagonal.    Symmetry  in  the  overall  algorithm  is  obtained  by 
using a weighted average of the values of 𝜙𝑗 calculated in elements 𝑗 + 1/2 and 𝑗 − 1/2. 
A  monotonic  element-centered  momentum  advection  algorithm  is  obtained  by 
choosing the identity matrix for the transformation and by using mass weighting for the 
inverse relationship. 
{⎧Ψ1,𝑗+1
}⎫
2⁄
2⁄ ⎭}⎬
⎩{⎨
Ψ2,𝑗+1
To conserve momentum, Ψ is advected with the transport masses. 
−
v𝑗
− } 
v𝑗+1
= [1
] {
(M
− Ψ
𝑗+1
−
𝑚,𝑗+1
+
Ψ𝑚,𝑗+1/2
=
+ Ψ𝑚,𝑗
− 𝑓 ̃
−
𝑗 − Ψ𝑚,𝑗+1
+
𝑗+1
𝑓 ̃
𝑗+1)
, 
(20.2.102)
(20.2.103)
v𝑗 =
2M𝑗
(M𝑗+1/2Ψ1,𝑗+1/2 + M𝑗−1/2Ψ2,𝑗−1/2).
(20.2.104)
Dispersion  Errors.  A  von  Neumann  analysis  [Trefethen  1982]  characterizes  the 
dispersion  errors  of  linear  advection  algorithms.    Since  the  momentum  advection 
the 
algorithm  modifies 
momentum  advection  algorithm  does  not  necessarily  have  the  same  dispersion 
characteristics as the underlying algorithm.  The von Neumann analysis provides a tool 
to explore the changes in the dispersion characteristics without considering a particular 
underlying advection algorithm.  
the  underlying  element-centered  advection  algorithm, 
The model problem is the linear advection equation with a constant value of c.  A 
class  of  solutions  can  be  expressed  as  complex  exponentials,  where  i  is  √−1  ,  ω  is  the 
frequency, and χ is the wave number. 
∂φ
∂𝑡
+ c
∂φ
∂𝑥
= 0,
φ(𝑥, 𝑡) = 𝑒𝑖(ω𝑡−χ𝑥).
(20.2.105)
(20.2.106)
For  Equation  (17.2.24),  the  dispersion  equation  is  𝜔 = 𝑐𝜒,  but  for  discrete 
approximations  of  the  equation  and  for  general  hyperbolic  equations,  the  relation  is 
𝜔 = 𝜔𝜒.    The  phase  velocity,  cp,  and  the  group  speed,  cg,  are  defined  by  Equation 
(17.2.25). 
cp =
,
(20.2.107)
Simplified Arbitrary Lagrangian-Eulerian 
LS-DYNA Theory Manual 
cg =
∂ω
.
∂χ
(20.2.108)
The mesh spacing is assumed to have a constant value 𝐽, and the time step, ℎ, is 
also constant.  The + and - states in the previous discussions correspond to times n and 
n + 1 in the dispersion analysis.  An explicit linear advection method that has the form 
given by Equation (1.2.109) results in a complex dispersion equation, Equation (17.2.27), 
where Π is a complex polynomial. 
𝑛+1 = 𝜑𝑗
𝜑𝑗
𝑛 + F(c, ℎ, 𝐽, . . . , 𝜑𝑗−1
𝑛 , 𝜑𝑗,
𝑛𝜑𝑗+1
𝑛 , . . . ),
𝑒𝑖ωℎ = 1 + P(𝑒𝑖χ𝐽),
Π(𝑒𝑖χ𝐽) = ∑ 𝛽𝑗𝑒𝑖χ𝑗𝐽
.
(20.2.109)
(20.2.110)
(20.2.111)
The dispersion equation has the general form given in Equation (1.2.112), where 
Πr and Πi denote the real and imaginary parts of Π, respectively. 
Π𝑖
1 + Πr
Recognizing  that  the  relations  in  the  above  equations  are  periodic  in  𝜔ℎ  and  χ𝐽,  the 
normalized frequency and wave number are defined to simplify the notation. 
ωℎ = tan−1 (
(20.2.112)
).
𝜔̅̅̅̅ = ωℎ,
χ̅̅̅̅ = χ𝐽.
(20.2.113)
The  von  Neumann  analysis  of  the  SALE  algorithm  proceeds  by  first  calculating  the 
increment in the cell momentum. 
p𝑗+1/2
=
(v𝑗
𝑛 + v𝑗+1
𝑛 ),
p𝑗+1/2
=
𝑛,
(1 + 𝑒−𝑖χ̅̅̅̅̅)v𝑗
Δp𝑗+1/2
𝑛+1 = P𝑗+1
2⁄
𝑛+1 − P𝑗+1
2⁄
,
Δp𝑗+1/2
𝑛+1 =
𝑛.
(1 + e−𝑖χ̅̅̅̅̅)Πv𝑗
The velocity is updated from the changes in the cell momentum. 
𝑛+1 = v𝑗
v𝑗
𝑛 +
(Δp𝑗+1/2
𝑛+1 + Δp𝑗−1/2
𝑛+1 ),
𝑛+1 =
v𝑗
𝑛,
(1 + 𝑒𝑖χ̅̅̅̅̅)(1 + 𝑒−𝑖χ̅̅̅̅̅)Πv𝑗
(20.2.114)
(20.2.115)
(20.2.116)
(20.2.117)
(20.2.118)
(20.2.119)
LS-DYNA Theory Manual 
Simplified Arbitrary Lagrangian-Eulerian 
𝑛+1 =
v𝑗
𝑛.
(1 + cos(χ̅̅̅̅))Πv𝑗
(20.2.120)
The  dispersion  relation  for  the  SALE  advection  algorithm  is  given  by  Equation 
(1.2.121). 
𝜔̅̅̅̅ = tan−1
⎜⎜⎜⎛
⎝
1 + 1
(1 + cos(χ̅̅̅̅))Π𝑖
⎟⎟⎟⎞
(1 + cos(χ̅̅̅̅))Πr⎠
. 
(20.2.121)
By comparing Equation (20.2.112) and Equation (20.2.121), the effect of the SALE 
momentum  advection  algorithm  on  the  dispersion  is  to  introduce  a  factor  λ,  equal  to 
2 (1 + cos(χ̅̅̅̅))Π, into the spatial part of the advection stencil.  For small values of χ̅̅̅̅, λ is 
close  to  one,  and  the  dispersion  characteristics  are  not  changed,  but  when  χ̅̅̅̅  is  π,  the 
phase and group velocity go to zero and the amplification factor is one independent of 
the  underlying  advection  algorithm.    Not  only  is  the  wave  not  transported,  it  is  not 
damped  out.    The  same  effect  is  found  in  two  dimensions,  where  λ,  has  the  form 
4 (1 + cos(χ̅̅̅̅) + cos(χ̅̅̅̅̅̅̅̅) + cos(χ̅̅̅̅)cos(χ̅̅̅̅̅̅̅̅)). 
In contrast, none of the other algorithms alter the dispersion characteristics of the 
underlying  algorithm.    Benson  has  demonstrated  for  the  element-centered  algorithms 
that the SALE inversion error and the dispersion problem are linked.  Algorithms that 
fall into the same general class as the SALE and HIS algorithms will, therefore, not have 
dispersion problems [Benson 1992]. 
Three-Dimensional  Momentum  Advection  Algorithms.    The  momentum  advection 
algorithms  discussed  in  the  previous  sections  are  extended  to  three  dimensions  in  a 
straightforward manner.  The staggered mesh algorithm requires the construction of a 
staggered  mesh  and  the  appropriate  transport  masses.    Based  on  the  consistency 
arguments, the appropriate transport masses are given by Equation (1.2.122).  
𝑓 ̃
𝑗+1/2,𝑘,𝑙 =
𝑙+1
2⁄
𝑘+1
2⁄
𝑗+1
∑ ∑ ∑ 𝑓𝐽,𝐾,𝐿
𝐽=𝑗
𝐾=𝑘−1
𝐿=𝑙−1
2⁄
2⁄
. 
(20.2.122)
The SALE advection algorithm calculates the average momentum of the element 
from the four velocities at the nodes and distributes 1⁄8 of the change in momentum to 
each node. 
p𝑗+1
2⁄ ,𝑘+1
2⁄ ,𝑙+1
2⁄ =
𝑗+1
𝑘+1
𝑙+1
𝜌𝑗+1
2⁄ ,𝑘+1
2⁄ ,𝑙+1
2⁄ ∑ ∑ ∑ v𝐽𝐾𝐿
𝐽=𝑗
𝐾=𝑘
𝐿=𝑙
, 
(20.2.123)
Simplified Arbitrary Lagrangian-Eulerian 
LS-DYNA Theory Manual 
p𝑗+1
2⁄ ,𝑘+1
2⁄ ,𝑙+1
2⁄ =
𝑗+1
𝑘+1
𝑙+1
𝑀𝑗+1
2⁄ ,𝑘+1
2⁄ ,𝑙+1
2⁄ ∑ ∑ ∑ v𝐽𝐾𝐿
𝐽=𝑗
𝐾=𝑘
𝐿=𝑙
, 
(20.2.124)
+ =
v𝑗,𝑘,𝑙
+
𝑀𝑗,𝑘,𝑙
⎜⎜⎜⎛
⎝
𝑀𝑗,𝑘,𝑙
− 𝑣𝑗,𝑘,𝑙
− +
2⁄
𝑘+1
𝑗+1
∑ ∑ ∑ 𝛥𝑃𝐽,𝐾,𝐿
𝑙+1
2⁄
2⁄
𝐽=𝑗−1
2⁄
𝐾=𝑘−1
2⁄
𝐿=𝑙−1
2⁄
. 
⎟⎟⎟⎞
⎠
(20.2.125)
The  HIS  algorithm  is  also  readily  extended  to  three  dimensions.    The  variable 
definitions are given in Equation (1.2.126) and Equation (1.2.127), where the subscript A 
refers to the local numbering of the nodes in the element.  In an unstructured mesh, the 
relative  orientation  of  the  nodal  numbering  within  the  elements  may  change.    The 
subscript A is always with reference to the numbering in element 𝑗, 𝑘, 𝑙.  The subscript à 
is  the  local  node  number  in  an  adjacent  element  that  refers  to  the  same  global  node 
number as A. 
ΨA,𝑗+1
2⁄ ,𝑘+1
2⁄ ,𝑙+1
2⁄ = vA,𝑗+1
2⁄ ,𝑘+1
2⁄ ,𝑙+1
2⁄ ,
+ =
v𝑗,𝑘,𝑙
2⁄
𝑗+1
𝑘+1
𝑙+1
+ ∑ ∑ ∑ MJ,K,LΨÃ,J,K,L
M𝑗,𝑘,𝑙
𝐿=𝑙−1
𝐾=𝑘−1
𝐽=𝑗−1
2⁄
2⁄
+
2⁄
2⁄
2⁄
(20.2.126)
. 
(20.2.127)
20.3  The Manual Rezone 
The  central  limitation  to  the  simplified  ALE  formulation  is  that  the  topology  of 
the mesh is fixed.  For a problem involving large deformations, a mesh that works well 
at early times may not work at late times regardless of how the mesh is distributed over 
the  material  domain.    To  circumvent  this  difficulty,  a  manual  rezoning  capability  has 
been  implemented  in  LS-DYNA.    The  general  procedure  is  to  1)  interrupt  the 
calculation  when  the  mesh  is  no  longer  acceptable,  2)  generate  a  new  mesh  with 
INGRID by using the current material boundaries from LS-DYNA (the topologies of the 
new and old mesh are unrelated), 3) remap the solution from the old mesh to the new 
mesh, and 4) restart the calculation.  
This  chapter  will  concentrate  on  the  remapping  algorithm  since  the  mesh 
generation  capability  is  documented  in  the  INGRID  manual  [Stillman  and  Hallquist 
1992].    The  remapping  algorithm  first  constructs  an  interpolation  function  on  the 
original mesh by using a least squares procedure, and then interpolates for the solution 
values on the new mesh.  
The  one  point  quadrature  used  in  LS-DYNA  implies  a  piecewise  constant 
distribution  of  the  solution  variables  within  the  elements.    A  piecewise  constant
LS-DYNA Theory Manual 
Simplified Arbitrary Lagrangian-Eulerian 
distribution  is  not  acceptable  for  a  rezoner  since  it  implies  that  for  even  moderately 
large  changes  in  the  locations  of  the  nodes  (say,  displacements  on  the  order  of  fifty 
percent of the elements characteristic lengths) that there will be no changes in the values 
of  the  element-centered  solution  variables.    A  least  squares  algorithm  is  used  to 
generate  values  for  the  solution  variables  at  the  nodes  from  the  element-centered 
values.    The  values  of  the  solution  variables  can  then  be  interpolated  from  the  nodal 
values, 𝜙A, using the standard trilinear shape functions anywhere within the mesh. 
𝜙(𝜉 , 𝜂, 𝜁 ) = 𝜙𝐴NA(𝜉 , 𝜂, 𝜁 ).
(20.3.128)
The  objective  function  for  minimization,  𝐽,  is  defined  material  by  material,  and 
each material is remapped independently. 
𝐽 =
∫(φA
NA − φ)2dV.
(20.3.129)
The objective function is minimized by setting the derivatives of 𝐽 with respect to 
𝜙𝐴 equal to zero. 
∂𝐽
∂φA
= ∫(φB
NB − φ)NAdV = 0.
(20.3.130)
The  least  square  values  of  𝜙A  are  calculated  by  solving  the  system  of  linear 
equations, Equation (17.3.4). 
MABφB = ∫ NA
φdV,
MAB = ∫ NA
NBdV.
(20.3.131)
(20.3.132)
The  “mass  matrix”,  MAB,  is  lumped  to  give  a  diagonal  matrix.    This  eliminates  the 
spurious  oscillations  that  occur  in  a  least  squares  fit  around  the  discontinuities  in  the 
solution (e.g., shock waves) and facilitates an explicit solution for 𝜙A.  The integral on 
the right hand side of Equation (20.3.131) is evaluated using one point integration.  By 
introducing  these  simplifications,  Equation (17.3.4)  is  reduced  to  Equation  (1.3.133), 
where the summation over a is restricted to the elements containing node A. 
φA =
∑ φαVα
∑ Vαα
.
(20.3.133)
The  value  of  𝜙α  is  the  mean  value  of  𝜙  in  element  a.    From  this  definition,  the 
value of 𝜙α is calculated using Equation (1.3.134). 
φα =
Vα
∫ φA
Vα
NAdV.
(20.3.134)
Simplified Arbitrary Lagrangian-Eulerian 
LS-DYNA Theory Manual 
The integrand in Equation (20.3.134) is defined on the old mesh, so that Equation 
(20.3.134) is actually performed on the region of the old mesh that overlaps element α in 
the new mesh, where the superscript “*” refers to elements on the old mesh. 
φα =
Vα
∑ ∗
∫ φA
NAdV∗.
∗
Vα∩Vβ
(20.3.135)
One  point  integration  is  currently  used  to  evaluate  Equation  (20.3.135),  although  it 
would  be  a  trivial  matter  to  add  higher  order  integration.    By  introducing  this 
simplification,  Equation  (20.3.135)  reduces  to  interpolating  the  value  of   𝜙𝛼  from  the 
least squares fit on the old mesh.  
𝜙a = 𝜙ANA(𝜉 ∗, 𝜂∗, 𝜁 ∗).
(20.3.136)
The  isoparametric  coordinates  in  the  old  mesh  that  correspond  to  the  spatial 
location  of  the  new  element  centroid  must  be  calculated  for  Equation  (20.3.136).    The 
algorithm that is described here is from Shapiro [1990], who references [Thompson and 
Maffeo 1985, Maffeo 1984, Maffeo 1985] as the motivations for his current strategy, and 
we follow his notation.  The algorithm uses a “coarse filter” and a “fine filter” to make 
the search for the correct element in the old mesh efficient. 
The  coarse  filter  calculates  the  minimum  and  maximum  coordinates  of  each 
element in the old mesh.  If the new element centroid, (𝑥𝑠, 𝑦𝑠, 𝑧𝑠), lies outside of the box 
defined by the maximum and minimum values of an old element, then the old element 
does not contain the new element centroid. 
Several  elements  may  pass  the  coarse  filter  but  only  one  of  them  contains  the 
new  centroid.    The  fine  filter  is  used  to  determine  if  an  element  actually  contains  the 
new  centroid.    The  fine  filter  algorithm  will  be  explained  in  detail  for  the  two-
dimensional  case  since  it  easier  to  visualize  than  the  three-dimensional  case,  but  the 
final equations will be given for the three-dimensional case. 
The two edges adjacent to each node in Figure 20.2 (taken from [Shapiro 1990]) 
define  four  skew  coordinate  systems.    If  the  coordinates  for  the  new  centroid  are 
positive  for  each  coordinate  system,  then  the  new  centroid  is  located  within  the  old 
element.  Because of the overlap of the four positive quarter spaces defined by the skew 
coordinate  systems,  only  two  coordinate  systems  actually  have  to  be  checked.    Using 
the first and third coordinate systems, the coordinates, α𝑖, are the solution of Equation 
(17.3.9). 
𝑉𝑠 = 𝑉1 + 𝑎1𝑉12 + 𝑎2𝑉14,
𝑉𝑠 = 𝑉3 + 𝑎3𝑉32 + 𝑎4𝑉34.
(20.3.137)
(20.3.138)
LS-DYNA Theory Manual 
Simplified Arbitrary Lagrangian-Eulerian 
3v32
(xs, ys)
1v12
v1
vs
4v34
2v14
Figure 20.2.  Skew Coordinate System 
Two  sets  of  linear  equations  are  generated  for  the  α𝑖  by  expanding  the  vector 
equations. 
[
𝑥2 − 𝑥1
𝑦2 − 𝑦1
𝑥4 − 𝑥1
𝑦4 − 𝑦1
] {
[
𝑥2 − 𝑥3
𝑦2 − 𝑦3
𝑥4 − 𝑥3
𝑦4 − 𝑦3
] {
𝛼1
𝛼2
𝛼3
𝛼4
} = {
𝑥𝑠 − 𝑥1
𝑦𝑠 − 𝑦1
} = {
𝑥𝑠 − 𝑥3
𝑦𝑠 − 𝑦3
},
}.
(20.3.139)
(20.3.140)
The generalization of Equation (17.3.9) to three dimensions is given by Equation 
(17.3.11),  and  it  requires  the  solution  of  four  sets  of  three  equations.    The  numbering 
convention for the nodes in Equation (17.3.11) follows the standard numbering scheme 
used in LS-DYNA for eight node solid elements. 
𝑉s = 𝑉1 + 𝑎1𝑉12 + 𝑎2𝑉14 + 𝑎3𝑉15,
𝑉s = 𝑉3 + 𝑎4𝑉37 + 𝑎5𝑉34 + 𝑎6𝑉32,
𝑉s = 𝑉6 + 𝑎7𝑉62 + 𝑎8𝑉65 + 𝑎9𝑉67,
𝑉s = 𝑉8 + 𝑎10𝑉85 + 𝑎11𝑉84 + 𝑎12𝑉87.
(20.3.141)
(20.3.142)
(20.3.143)
(20.3.144)
The  fine  filter  sometimes  fails  to  locate  the  correct  element  when  the  mesh  is 
distorted.  When this occurs, the element that is closest to the new centroid is located by 
finding  the element  for  which  the  sum  of  the  distances  between  the  new  centroid  and 
the nodes of the element is a minimum.
Simplified Arbitrary Lagrangian-Eulerian 
LS-DYNA Theory Manual 
Once  the  correct  element  is  found,  the  isoparametric  coordinates  are  calculated 
using the Newton-Raphson method, which usually converges in three or four iterations. 
𝑦A
⎡𝑥A
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
𝑧A
∂𝑁A
∂𝜉
∂𝑁A
∂𝜉
∂𝑁A
∂𝜉
𝑥A
𝑦A
𝑧A
∂𝑁A
∂𝜂
∂𝑁A
∂𝜂
∂𝑁A
∂𝜂
𝑥A
𝑦A
𝑧A
∂𝑁A
⎤
∂𝜁
⎥
⎥
∂𝑁A
⎥
⎥
∂𝜁
⎥
⎥
∂𝑁A
⎥
∂𝜁 ⎦
{⎧Δ𝜉
}⎫
Δ𝜂
Δ𝜁 ⎭}⎬
⎩{⎨
=
{⎧𝑥s − 𝑥A𝑁A
}⎫
𝑦s − 𝑦A𝑁A
, 
𝑧s − 𝑧A𝑁A ⎭}⎬
⎩{⎨
𝜉 𝑖+1 = 𝜉 𝑖 + 𝛥𝜉 , 
𝜂𝑖+1 = 𝜂𝑖 + 𝛥𝜂, 
𝜁 𝑖+1 = 𝜁 𝑖 + 𝛥𝜁 .
(20.3.145)
(20.3.146)
LS-DYNA Theory Manual 
Stress Update Overview 
21    
Stress Update Overview 
21.1  Jaumann Stress Rate 
Stresses  for  material  which  exhibit  elastic-plastic  and  soil-like  behavior 
(hypoelastic) are integrated incrementally in time: 
𝜎𝑖𝑗(𝑡 + 𝑑𝑡) = 𝜎𝑖𝑗(𝑡) + 𝜎̇𝑖𝑗𝑑𝑡,
(21.1)
Here, and in equations which follow, we neglect the contribution of the bulk viscosity to 
the stress tensor.  In Equation (21.1), the dot denotes the material time derivative given 
by 
in which 
is the spin tensor and 
𝜎̇𝑖𝑗 = 𝜎𝑖𝑗
∇ + 𝜎𝑖𝑘𝜔𝑘𝑗 + 𝜎𝑗𝑘𝜔𝑘𝑖,
𝜔𝑖𝑗 =
(
∂𝑣𝑖
∂𝑥𝑗
−
∂𝑣𝑗
∂𝑥𝑖
),
∇ = 𝐶𝑖𝑗𝑘𝑙𝜀̇𝑘𝑙,
𝜎𝑖𝑗
(21.2)
(21.3)
(21.4)
is the Jaumann (co-rotational) stress rate.  In Equation (21.4), 𝐶𝑖𝑗𝑘𝑙 is the stress dependent 
constitutive matrix, 𝑣𝑖, is the velocity vector, and 𝜀̇𝑖𝑗 is the strain rate tensor: 
𝜀̇𝑖𝑗 =
(
∂𝑣𝑖
∂𝑥𝑗
+
∂𝑣𝑗
∂𝑥𝑖
).
(21.5)
In  the  implementation  of  Equation  (21.1)  we  first  perform  the  stress  rotation, 
Equation  (21.2),  and  then  call  a  constitutive  subroutine  to  add  the  incremental  stress 
components 𝜎𝑖𝑗
𝛻 .  This may be written as  
𝑛+1 = 𝜎𝑖𝑗
𝜎𝑖𝑗
𝑛 + 𝑟𝑖𝑗
𝑛 + 𝜎𝑖𝑗
𝛻𝑛+1
2⁄
Δ𝑡𝑛+1
2⁄ ,
(21.6)
Stress Update Overview 
LS-DYNA Theory Manual 
where 
𝛻𝑛+1
2⁄
𝜎𝑖𝑗
𝑛+1
2⁄
Δ𝜀𝑖𝑗
𝑛+1
2⁄
Δ𝑡𝑛+1
2⁄ = 𝐶𝑖𝑗𝑘𝑙Δ𝜀𝑘𝑙
𝑛+1
Δ𝑡𝑛+1
2⁄
2⁄ ,
= 𝜀̇𝑖𝑗
, 
and 𝑟𝑖𝑗
𝑛 gives the rotation of the stress at time 𝑡𝑛 to the configuration at 𝑡𝑛 + 1 
𝑛 = (𝜎𝑖𝑝
𝑟𝑖𝑗
𝑛 𝜔𝑝𝑗
𝑛+1
2⁄
+ 𝜎𝑗𝑝
𝑛 𝜔𝑝𝑖
𝑛+1
2⁄
) Δ𝑡𝑛+1
2⁄ .
(21.7)
(21.8)
In  the  implicit  NIKE2D/3D  [Hallquist  1981b]  codes,  which  are  used  for  low 
frequency  structural  response,  we  do  a  half-step  rotation,  apply  the  constitutive  law, 
and  complete  the  second  half-step  rotation  on  the  modified  stress.    This  approach  has 
also  been  adopted  for  some  element  formulations  in  LS-DYNA  when  the  invariant 
stress update is active.  An exact or second order accurate rotation is performed rather 
than the approximate one represented by Equation (21.3), which is valid only for small 
incremental rotations.  A typical implicit time step is usually 100 to 1000 or more times 
larger than the explicit time step; consequently, the direct use of  Equation (21.7) could 
lead to very significant errors. 
21.2  Jaumann Stress Rate Used With Equations of State 
If pressure is defined by an equation of state as a function of relative volume, 𝑉, 
and energy, 𝐸, or temperature, 𝑇, 
we update the deviatoric stress components 
𝑝 = 𝑝(𝑉, 𝐸) = 𝑝(𝑉, 𝑇),
𝑛+1
2⁄
where 𝜀̇′𝑖𝑗
𝑛+1 = 𝜎𝑖𝑗
𝑠𝑖𝑗
𝑛 + 𝑟𝑖𝑗
𝑛 + 𝑝𝑛𝛿𝑖𝑗 + 𝐶𝑖𝑗𝑘𝑙𝜀̇′𝑘𝑙
𝑛+1
2⁄
 is the deviatoric strain rate tensor: 
𝑛+1
2⁄
𝜀̇′𝑖𝑗
= 𝜀̇𝑖𝑗 −
𝜀̇𝑘𝑘𝛿.
𝛥𝑡𝑛+1
2⁄ ,
(21.9)
(21.10)
(21.11)
Before the equation of state, Equation (21.9), is evaluated, we  compute the bulk 
viscosity, 𝑞, and update the total internal energy 𝑒 of the element being processed to a 
trial value 𝑒∗: 
𝑒∗𝑛+1 = 𝑒𝑛 −
Δ𝑣 (𝑝𝑛 + 𝑞𝑛−1
2⁄ + 𝑞𝑛+1
2⁄ ) + 𝑣𝑛+1
𝑛+1
2⁄
2⁄ 𝑠𝑖𝑗
𝑛+1
2⁄
Δ𝜀𝑖𝑗
, 
(21.12)
where 𝑣 is the element volume and
LS-DYNA Theory Manual 
Stress Update Overview 
Δ𝑣 = 𝑣𝑛+1 − 𝑣𝑛,      𝑣𝑛+1
The time-centering of the viscosity is explained by Noh [1976]. 
(𝑣𝑛 + 𝑣𝑛+1),
2⁄ =
2 =
𝑛+1
𝑠𝑖𝑗
(𝑠𝑖𝑗
𝑛 + 𝑠𝑖𝑗
𝑛+1). 
(21.13)
Assume we have an equation of state that is linear in internal energy of the form 
where 
𝑝𝑛+1 = 𝐴𝑛+1 + 𝐵𝑛+1𝐸𝑛+1,
𝐸𝑛+1 =
𝑒𝑛+1
𝑣0
,
and 𝜐0 is the initial volume of the element.  Noting that 
𝑒𝑛+1 = 𝑒∗𝑛+1 −
Δ𝑣𝑝𝑛+1,
pressure can be evaluated exactly by solving the implicit form 
𝑝𝑛+1 =
(𝐴𝑛+1 + 𝐵𝑛+1𝐸∗𝑛+1)
, 
(1 + 1
𝐵𝑛+1 Δ𝑣
𝑣0
)
(21.14)
(21.15)
(21.16)
(21.17)
and the internal energy can be  updated in Equation (21.16).  If the equation of state is 
not linear in internal energy, a one-step iteration is used to approximate the pressure 
𝑝∗𝑛+1 = 𝑝(𝑉𝑛+1, 𝐸∗𝑛+1).
(21.18)
Internal  energy  is  updated  to  𝑛 + 1  using  𝑝∗𝑛+1  in  Equation  (21.16)  and  the  final 
pressure is then computed: 
𝑝𝑛+1 = 𝑝(𝑉𝑛+1, 𝐸𝑛+1).
(21.19)
This is also the iteration procedure used in KOVEC [Woodruff 1973].  All the equations 
of state in LS-DYNA are linear in energy except the ratio of polynomials. 
21.3  Green-Naghdi Stress Rate 
The Green-Naghdi rate is defined as 
𝛻 = 𝜎̇𝑖𝑗 + 𝜎𝑖𝑘𝛺𝑘𝑗 + 𝜎𝑗𝑘𝛺𝑘𝑖 = 𝑅𝑖𝑘𝑅𝑗𝑙𝜏̇
𝜎𝑖𝑗
,
𝑘𝑙
where 𝛺𝑖𝑗 is defined as 
𝛺𝑖𝑗 = 𝑅̇ 𝑖𝑘𝑅𝑖𝑘,
and 𝐑 is found by application of the polar decomposition theorem 
𝐹𝑖𝑗 = 𝑅𝑖𝑘𝑈𝑘𝑗 = 𝑉𝑖𝑘𝑅𝑘𝑗,
(21.20)
(21.21)
(21.22)
Stress Update Overview 
LS-DYNA Theory Manual 
𝐹𝑖𝑗 is the deformation gradient matrix and 𝑈𝑖𝑗 and 𝑉𝑖𝑗 are the positive definite right and 
left stretch tensors: 
𝐹𝑖𝑗 =
𝜕𝑥𝑖
𝜕𝑋𝑗
.
(21.23)
Stresses  are  updated  for  all  materials  by  adding  to  the  rotated  Cauchy  stress  at 
time n. 
the stress increment obtained by an evaluation of the constitutive equations, 
𝑛 = 𝑅𝑘𝑖
𝜏𝑖𝑗
𝑛 𝑅𝑙𝑗
𝑛,
𝑛𝜎𝑘𝑙
𝑛+1
2⁄
Δ𝜏𝑖𝑗
where 
= 𝐶𝑖𝑗𝑘𝑙 Δ𝑑𝑘𝑙
𝑛+1
2⁄
,
𝑛+1
2⁄
Δ𝑑𝑖𝑗
𝑛+1
2⁄
= 𝑅𝑘𝑖
𝑛+1
2⁄
𝑅𝑙𝑗
𝑛+1
2⁄
Δ𝜀𝑘𝑙
𝐶𝑖𝑗𝑘𝑙 
Δ𝜀𝑘𝑙 
 =  
 =  
constitutive matrix 
increment in strain 
and to obtain the rotated Cauchy stress at 𝑡𝑛+1, i.e.,  
𝑛+1 = 𝜏𝑖𝑗
𝜏𝑖𝑗
𝑛 + Δ𝜏𝑖𝑗
𝑛+1
2⁄
.
The desired Cauchy stress at 𝑛 + 1 can now be found 
𝑛+1 = 𝑅𝑖𝑘
𝜎𝑖𝑗
𝑛+1𝑅𝑗𝑙
𝑛+1𝜏𝑘𝑙
𝑛+1.
(21.24)
(21.25)
(21.26)
(21.27)
(21.28)
Because we evaluate our constitutive models in the rotated configuration, we avoid the 
need  to  transform  history  variables  such  as  the  back  stress  that  arises  in  kinematic 
hardening. 
In the computation of 𝐑, Taylor and Flanagan [1989] did an incremental update 
in  contrast  with  the  direct  polar  decomposition  used  in  the  NIKE3D  code.    Following 
their notation the algorithm is given by.
LS-DYNA Theory Manual 
Stress Update Overview 
𝑧𝑖 = 𝑒𝑖𝑗𝑘𝑉𝑗𝑚𝜀̇𝑚𝑘, 
𝜛𝑖 = 𝑒𝑖𝑗𝑘𝜔𝑗𝑘 − 2[𝑉𝑖𝑗 − 𝛿𝑖𝑗𝑉𝑘𝑘]
−1
𝑧𝑗, 
𝛺𝑖𝑗 =
𝑒𝑖𝑗𝑘𝜛𝑘, 
𝛥𝑡
𝛺𝑖𝑘) 𝑅𝑘𝑗
𝛥𝑡
𝑛+1 = (𝛿𝑖𝑘 +
(𝛿𝑖𝑘 −
𝑉̇𝑖𝑗 = (𝜀̇𝑖𝑘 + 𝜔𝑖𝑘)𝑉𝑘𝑗 − 𝑉𝑖𝑘𝛺𝑘𝑗, 
𝑛 + 𝛥𝑡𝑉̇𝑖𝑗. 
𝑉𝑖𝑗
𝑛+1 = 𝑉𝑖𝑗
𝑛 , 
𝛺𝑖𝑘) 𝑅𝑘𝑗
(21.29)
We  have  adopted  the  PRONTO3D  approach  in  LS-DYNA  due  to  numerical 
difficulties  with  the  polar  decomposition  in  NIKE3D.    We  believe  the  PRONTO3D 
approach is reliable.  Several disadvantages of the PRONTO3D approach include 300+ 
operations  (at  least  that  is  the  number  we  got),  the  requirement  of  15  additional 
variables  per  integration  point,  and  if  we  rezone  the  material  in  the  future  the  initial 
geometry will need to be remapped and the 15 variables initialized. 
21.4  Elastoplastic Materials 
At  low  stress  levels  in  elastoplastic  materials  the  stresses,  𝜎𝑖𝑗,  depends  only  on 
the  state  of  strain;  however,  above  a  certain  stress  level,  called  the  yield  stress,  𝜎𝑦(𝑎𝑖), 
Initial uniaxial
yield point σ
y0
y = σ
experimental curve
y(ai)
L0
plastic strain
ε = ln(L/L0)
σ = P/A
elastic
strain
Figure 21.1.  The uniaxial tension test demonstrates plastic behavior.
Stress Update Overview 
LS-DYNA Theory Manual 
yield surface
defined by
F(δ
ij, k)
1 = σ
2 = σ
deviatoria plane
yield curve = intersection of the deviatoric
plane with the yield surface
  The  yield  surface  in  principal  stress  space  in  pressure
Figure  21.2. 
independent. 
nonrecoverable  plastic  deformations  are  obtained.    The  yield  stress  changes  with 
increasing plastic deformations, which are measured by internal variables, 𝑎𝑖. 
In  the  uniaxial  tension  test,  a  curve  like  that  in  Figure  21.1  is  generated  where 
logrithmic uniaxial strain is plotted against the uniaxial true stress which is defined as 
the applied load 𝑃 divided by the actual cross-sectional area, 𝐴.   
For  the  simple  von  Mises  plasticity  models  the  yield  stress  is  pressure 
independent  and  the  yield  surface  is  a  cylinder  in  principal  stress  space  as  shown  in 
Figure 21.2.  With isotropic hardening the diameter of the cylinder grows but the shape 
remains  circular.    In  kinematic  hardening  the  diameter  may  remain  constant  but  will 
translate in the plane as a function of the plastic strain tensor, See Figure 21.3. 
The equation describing the pressure independent yield surface, 𝐹, is a function 
of the deviatoric stress tensor, 𝑠𝑖𝑗, of a form given in Equation (1.30). 
𝐹(𝑠𝑖𝑗, 𝑎𝑖) = 𝑓 (𝑠𝑖𝑗) − 𝜎𝑦(𝑎𝑖) = 0,
(21.30)
𝑓 (𝑠𝑖𝑗) = determines the shape, 
𝜎𝑦(𝑎𝑖) = determines the translation and size. 
The existence of a potential function, 𝑔, called the plastic potential, is assumed 
Stability and uniqueness require that: 
𝑔 = 𝑔(𝑠𝑖𝑗).
p = 𝜆
𝑑𝜀𝑖𝑗
𝜕𝑔
𝜕𝑠𝑖𝑗
,
(21.31)
(21.32)
LS-DYNA Theory Manual 
Stress Update Overview 
initial yield
curve in the
deviatoric
plane
current
yield
surface
Figure  21.3.    With  kinematic  hardening  the  yield  surface  may  shift  as  a
function of plastic strain. 
where 𝜆 is a proportionality constant. 
As  depicted  in  Figure  21.5  the  plastic  strain  increments  𝑑𝜀𝑖𝑗
p  are  normal  to  the 
plastic potential function.  This is the normality rule of plasticity. 
The plastic potential 𝑔 is identical with the yield condition 𝐹(𝑠𝑖𝑗) 
Hence: 
𝑔 ≡ 𝐹.
𝑝 = 𝜆
𝑑𝜀𝑖𝑗
𝜕𝑓
𝜕𝑠𝑖𝑗
= 𝜆 grad𝑓
and the stress increments 𝑑𝑠𝑖𝑗 are normal to the plastic flow 
∂𝑔
∂s𝑖𝑗
. 
(21.33)
(21.34)
Post-yielding  behavior  from  uniaxial  tension  tests  typically  show  the  following 
behaviors illustrated in Figure 21.4: 
The  behavior  of  these  hardening  laws  are  characterized  in  Table  1.1.  below.  
Although LS-DYNA permits softening to be defined and used, such softening behavior 
will result in strain localization and nonconvergence with mesh refinement.
Stress Update Overview 
LS-DYNA Theory Manual 
(cid:1) 
(cid:1)
(cid:1)0
hardening
(cid:1) 
(cid:1)
(cid:1)0
(cid:2)
(cid:1) 
(cid:1)
(cid:1)0
ideal
(cid:2)
(cid:2)
softening
Figure 21.4.  Hardening, ideal, and softening plasticity models. 
Hardening 
Ideal 
Softening 
Behavior 
Stability 
Uniqueness 
Applications 
𝜎𝑦(𝑎𝑖) 
monotonic 
increasing 
yes 
yes 
is 
𝜎𝑦(𝑎𝑖) is constant 
is 
𝜎𝑦(𝑎𝑖) 
monotonic 
decreasing 
yes 
yes 
No 
No 
metals, 
concrete, 
with 
deformations 
rock 
small 
crude  idealization 
for  steel,  plastics, 
etc. 
dense sand, 
concrete with  
large 
deformations 
Table 21.1.  Plastic hardening, ideal plasticity, and softening. 
21.5  Hyperelastic Materials 
Stresses 
independent; 
for  elastic  and  hyperelastic  materials  are  path 
consequently, the stress update is not computed incrementally.  The methods described 
here are well known and the reader is referred to Green and Adkins [1970] and Ogden 
[1984] for more details. 
A  retangular  cartesian  coordinate  system  is  used  so  that  the  covariant  and  con-
travariant  metric  tensors  in  the  reference  (undeformed)  and  deformed  configuration 
are: 
𝐺𝑖𝑗 =
𝑔𝑖𝑗 = 𝑔𝑖𝑗 = 𝛿𝑖𝑗,
𝜕𝑥𝑘
𝜕𝑥𝑘
𝜕𝑋𝑗
𝜕𝑋𝑖
𝜕𝑋𝑗
𝜕𝑋𝑖
𝜕𝑥𝑘
𝜕𝑥𝑘
𝐺𝑖𝑗 =
.
, 
(21.35)
LS-DYNA Theory Manual 
Stress Update Overview 
The  Green-St.    Venant  strain  tensor  and  the  principal  strain  invariants  are 
defined as 
𝛾𝑖𝑗 =
(𝐺𝑖𝑗 − 𝛿𝑖𝑗),
𝐼1 = 𝛿𝑖𝑗𝐺𝑖𝑗,
𝐼2 =
𝐼3 = det(𝐺𝑖𝑗),
(𝛿𝑖𝑟𝛿𝑗𝑠𝐺𝑟𝑖𝐺𝑠𝑗 − 𝛿𝑖𝑟𝛿𝑗𝑠𝐺𝑖𝑗𝐺𝑟𝑠), 
(21.36)
(21.37)
For  a  compressible  elastic  material  the  existence  of  a  strain  energy  functional,  𝑊,  is 
assumed  
𝑊 = 𝑊(𝐼1, 𝐼2, 𝐼3),
(21.38)
which  defines  the  energy  per  unit  undeformed  volume.    The  stress  measured  in  the 
deformed configuration is given as [Green and Adkins, 1970]: 
(cid:4)  
(cid:1)(cid:2)(cid:3)
(cid:1)
Figure 21.5.  The plastic strain is normal to the yield surface. 
𝑠𝑖𝑗 = 𝛷𝑔𝑖𝑗 + 𝛹𝐵𝑖𝑗 + 𝑝𝐺𝑖𝑗, 
where  
,
𝛷 =
𝛹 =
√𝐼3
𝜕𝑊
𝜕𝐼1
𝜕𝑊
𝜕𝐼2
𝜕𝑊
𝑝 = 2√𝐼3
𝜕𝐼3
𝐵𝑖𝑗 = 𝐼1𝛿𝑖𝑗 − 𝛿𝑖𝑟𝛿𝑗𝑠𝐺𝑟𝑠.
√𝐼3
, 
, 
(21.39)
(21.40)
Stress Update Overview 
LS-DYNA Theory Manual 
This stress is related to the second Piola-Kirchhoff stress tensor: 
Second Piola-Kirchhoff stresses are transformed to physical (Cauchy) stresses according 
to the relationship: 
𝑆𝑖𝑗 = 𝑠𝑖𝑗√𝐼3.
(21.41)
𝜎𝑖𝑗 =
𝜌0
𝜕𝑥𝑖
𝜕𝑋𝑘
𝜕𝑥𝑗
𝜕𝑋𝑙
𝑆𝑘𝑙.
(21.42)
21.6  Layered Composites 
The composite models for shell elements in LS-DYNA include models for elastic 
behavior and inelastic behavior.  The approach used here for updating the stresses also 
applies to the airbag fabric model. 
To  allow  for  an  arbitrary  orientation  of  the  shell  elements  within  the  finite 
element  mesh,  each  ply  in  the  composite  has  a  unique  orientation  angle,  𝛽,  which 
measures the offset from some reference in the element.  Each integration point through 
the  shell  thickness,  typically  though  not  limited  to  one  point  per  ply,  requires  the 
definition of 𝛽 at that point.  The reference is determined by the angle 𝛹, which can be 
defined  for  each  element  on  the  element  card,  and  is  measured  from  the  1-2  element 
side. Figures 21.6 and 21.7 depict these angles.  
We update the stresses in the shell in the local shell coordinate system which is 
defined  by  the  1-2  element  side  and  the  cross  product  of  the  diagonals.    Thus  to 
transform the stress tensor into local system determined by the fiber directions entails a 
transformation that takes place in the plane of the shell. 
In the implementation of the material model we first transform the Cauchy stress 
and  velocity  strain  tensor 𝑑𝑖𝑗into  the  coordinate  system  of  the  material  denoted  by  the 
subscript L 
𝛔L =
𝛔L = 𝐪T𝛔𝐪,
𝐪L = 𝐪T𝐝𝐪, 
𝜎11 𝜎12 𝜎13
⎥⎤ , 
⎢⎡
𝜎21 𝜎22 𝜎23
𝜎32 𝜎32 𝜎33⎦
⎣
𝑑12
𝑑11
⎡
𝑑22
𝑑21
⎢
𝑑32
𝑑32
⎣
𝑑13
⎤
𝑑23
, 
⎥
𝑑33⎦
 𝛆L =
(21.43)
LS-DYNA Theory Manual 
Stress Update Overview 
θ = ψ+β
Figure 21.7.  A multi-layer laminate can be defined.  The angle βi is defined for 
the ith lamina. 
The Arabic subscripts on the stress and strain (𝛔 and 𝛆) are used to indicate the 
principal  material  directions  where  1  indicates  the  fiber  direction  and  2  indicates  the 
transverse fiber direction (in the plane).  The orthogonal 3 × 3 transformation matrix is 
given by 
𝐪 =
cos𝜃 −sin𝜃
⎢⎡
cos𝜃
sin𝜃
⎣
⎥⎤.
1⎦
(21.44)
In shell theory we assume a plane stress condition, i.e., that the normal stress, 𝜎33, to the 
mid-surface is zero.  We can now  incrementally update the stress state in the material 
coordinates 
𝑛+1 = 𝛔L
𝛔L
𝑛 + Δ𝛔L
𝑛+1
2⁄
,
(21.45)
where for an elastic material  
n4
n2
n3
n1
Figure 21.6.  Orientation of material directions relative to the 1-2 side.
Stress Update Overview 
LS-DYNA Theory Manual 
𝑛+1
2⁄
Δ𝛔L
=
Δ𝜎11
⎤
⎡
Δ𝜎22
⎥
⎢
⎥
⎢
Δ𝜎12
⎥
⎢
Δ𝜎23
⎥
⎢
Δ𝜎31⎦
⎣
=
𝑄11 𝑄12
⎡
𝑄12 𝑄22
⎢
⎢
⎢
⎢
⎣
𝑄44
𝑄55
⎤
⎥
⎥
⎥
⎥
𝑄66⎦
𝑑11
⎤
𝑑22
⎥
⎥
𝑑12
⎥
𝑑23
⎥
𝑑31⎦
⎡
⎢
⎢
⎢
⎢
⎣
Δ𝑡. 
(21.46)
The terms 𝑄𝑖𝑗 are referred to as reduced components of the lamina and are defined as 
,
, 
, 
(21.47)
𝑄11 =
𝑄22 =
𝑄12 =
𝐸11
1 − 𝜈12𝜈21
𝐸22
1 − 𝜈12𝜈21
𝜈12𝐸11
1 − 𝜈12𝜈21
𝑄44 = 𝐺12, 
𝑄55 = 𝐺23, 
𝑄66 = 𝐺31. 
Because of the symmetry properties,  
𝐸𝑗𝑗
𝐸𝑖𝑖
where  𝜈𝑖𝑗  is  Poisson’s  ratio  for  the  transverse  strain  in  jth  direction  for  the  material 
undergoing  stress  in  the  ith-direction, 𝐸𝑖𝑗  are  the  Young’s  modulii  in  the  ith  direction, 
and 𝐺𝑖𝑗 are the shear modulii. 
𝜈𝑗𝑖 = 𝜈𝑖𝑗
(21.48)
,
After  completion  of  the  stress  update  we  transform  the  stresses  back  into  the 
local shell coordinate system. 
𝛔 = 𝐪𝛔L𝐪T.
(21.49)
21.7  Constraints on Orthotropic Elastic Constants 
The inverse of the constitutive matrix 𝐂l is generally defined in terms of the local 
material  axes  for  an  orthotropic  material  is  given  in  terms  of  the  nine  independent 
elastic constants as
LS-DYNA Theory Manual 
Stress Update Overview 
−1 =
𝐂l
𝐸 11
𝜐 12
𝐸 11
𝜐 13
𝐸 11
−
−
−
𝜐 21
𝐸 22
𝐸 22
𝜐 23
𝐸 22
−
−
−
𝜐 31
𝐸 33
𝜐 32
𝐸 33
𝐸 33
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
𝐺12
𝐺23
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
. 
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
𝐺31⎦
(21.50)
As  discussed  by  Jones  [1975],  the  constants  for  a  thermodynamically  stable 
material must satisfy the following inequalities: 
𝐸1, 𝐸2, 𝐸3, 𝐺12, 𝐺23, 𝐺31 > 0,
𝐶11,𝐶22, 𝐶33, 𝐶44, 𝐶55, 𝐶66 > 0, 
(1 − 𝜈23𝜈32),
(1 − 𝜈13𝜈31),
1 − 𝜈12𝜈21 − 𝜈23𝜈32 − 𝜈31𝜈13 − 2𝜈21𝜈32𝜈13 > 0.
(1 − 𝜈12𝜈21) > 0, 
Using Equation (21.48) and (21.51) leads to: 
|𝜈21| < (
    |𝜈12| < (
∣𝜈32∣ < (
    ∣𝜈23∣ < (
∣𝜈13∣ < (
∣𝜈31∣ < (
2⁄
)
2⁄
)
2⁄
)
𝐸22
𝐸11
𝐸33
𝐸22
𝐸11
𝐸33
, 
, 
2⁄
)
2⁄
)
)
2⁄
.
𝐸11
𝐸22
𝐸22
𝐸33
𝐸33
𝐸11
(21.51)
(21.52)
21.8  Local Material Coordinate Systems in Solid Elements 
In  solid  elements  there  is  a  number  of  different  ways  of  defining  a  local 
coordinate system.  Perhaps the most general is by defining a triad for each element that 
is oriented in the local material directions, See Figure 21.8.  In this approach two vectors 
𝐚 and 𝐝 are defined.  The local 𝐜 direction is found from the cross product, 𝐜 = 𝐚 × 𝐝, the 
local  𝐛  direction  is  the  cross  product  𝐛 = 𝐜 × 𝐚.    This  triad  is  stored  as  history  data  at 
each integration point.
Stress Update Overview 
LS-DYNA Theory Manual 
Figure  21.8.    Local  material  directions  are  defined  by  a  triad  which  can  be 
input for each solid element. 
The  biggest  concern  when  dealing  with  local  material  directions  is  that  the 
results are not invariant with element numbering since the orientation of the local triad 
is  fixed  with  respect  to  the  base  of  the  brick  element,  nodes  1-4,  in  Figure  21.9.    For 
Hyperelastic materials where the stress tensor is computed in the initial configuration, 
this  is  not  a  problem,  but  for  materials  like  the  honeycomb  foams,  the  local  directions 
can  change  due  to  element  distortion  causing  relative  movement  of  nodes  1-4.    In 
honeycomb  foams  we  assume  that  the  material  directions  are  orthogonal  in  the 
deformed  configuration  since  the  stress  update  is  performed  in  the  deformed 
configuration.   
21.9  General Erosion Criteria for Solid Elements 
Several erosion criteria are available that are independent of the material models.  
Each one is applied independently, and once any one of them is satisfied, the element is 
deleted from the calculation.  The criteria for failure are: 
•  𝑃 ≥ 𝑃min  where  P  is  the  pressure  (positive  in  compression),  and  𝑃min  is  the 
pressure at failure. 
•  𝜎1 ≥ 𝜎max, where 𝜎1 is the maximum principal stress, and  𝜎max is the principal 
stress at failure. 
•  √3
′ 𝜎𝑖j
2 𝜎𝑖𝑗
′ ≥ 𝜎̅̅̅̅̅max, where 𝜎𝑖𝑗
equivalent stress at failure. 
′  are the deviatoric stress components, and 𝜎̅̅̅̅̅max is the 
•  𝜀1 ≥ 𝜀max,  where  𝜀1  is  the  maximum  principal  strain,  and  𝜀max  is  the  principal 
strain at failure. 
•  𝛾1 ≥ 𝛾max, where 𝛾1 is the shear strain, and 𝛾max is the shear strain at failure. 
•  The Tuler-Butcher criterion,
LS-DYNA Theory Manual 
Stress Update Overview 
Figure  21.9.    The  orientation  of  the  triad  for  the  local  material  directions  is
stored relative to the base of the solid element.  The base is defined by nodes 1-
4 of the element connectivity. 
∫ [max(0, 𝜎1 − 𝜎0)]2𝑑𝑡
≥ 𝐾f,
(21.53)
where 𝜎1 is the maximum principal stress, 𝜎0 is a specified threshold stress, 𝜎1 ≥ 𝜎0 ≥ 0, 
and 𝐾f is the stress impulse for failure.  Stress values below the threshold value are too 
low to cause fracture even for very long duration loadings.  Typical constants are given 
in Table 1.2 below [Rajendran, 1989]. 
These failure models apply to solid elements with one point integration in 2 and 
3 dimensions. 
Material 
1020 Steel 
OFHC Copper 
C1008 
HY100 
7039-T64 
𝜎0  (Kbar) 
10.0 
3.60 
14.0 
15.7 
8.60 
2 
2 
2 
2 
2 
12.5 
10.0 
0.38 
61.0 
3.00 
Table 21.2.  Typical constants for the Tuler-Bucher criterion. 
21.10  Strain Output to the LS-DYNA Database 
The strain tensors that are output to the LS-DYNA database from the solid, shell, 
and beam elements are integrated in time.   These strains are similar to the logarithmic 
strain  measure  and  are  based  on  an  integration  of  the  strain  rate  tensor.    Admittedly,
Stress Update Overview 
LS-DYNA Theory Manual 
the shear strain components do not integrate as logarithmic strain measures, but in spite 
of this, we have found that the strains output from LS-DYNA are far more useful than 
those  computed  in  LS-DYNA.    The  time  integration  of  the  strain  tensor  in  LS-DYNA 
maintains  objectivity  in  the  sense  that  rigid  body  motions  do  not  cause  spurious 
straining.   
Recall,  the  spin  tensor  and  strain  rate  tensor,  Equations  (21.3)  and  (21.5), 
respectively: 
𝜔𝑖𝑗 =
𝜀̇𝑖𝑗 =
(
𝜕𝑣𝑖
𝜕𝑥𝑗
−
𝜕𝑣𝑗
𝜕𝑥𝑖
),
(
𝜕𝑣𝑖
𝜕𝑥𝑗
+
𝜕𝑣𝑗
𝜕𝑥𝑖
).
In updating the strains from time 𝑛 to 𝑛 + 1, the following formula is used: 
𝑛+1 = 𝜀𝑖𝑗
𝜀𝑖𝑗
𝑛 + 𝜌𝑖𝑗
𝑛 + 𝜀̇𝑖𝑗
𝑛+1
2⁄
Δ𝑡𝑛+1
2⁄ ,
(21.54)
(21.55)
(21.56)
𝑛 gives the rotational correction that transforms the strain tensor at time 𝑡𝑛 into 
where 𝜌𝑖𝑗
the configuration at 𝑡𝑛 + 1 
𝑛 = (𝜀𝑖𝑝
𝜌𝑖𝑗
𝑛 𝜔𝑝𝑗
𝑛+1
2⁄
𝑛+1
+ 𝜀𝑗𝑝
𝑛 𝜔𝑝𝑖
2⁄
) Δ𝑡𝑛+1
2⁄ .
(21.57)
For  shell  elements  we  integrate  the  strain  tensor  at  the  inner  and  outer 
integration  points  and  output  two  tensors  per  element.    When  the  mid  surface  strains 
are plotted in LS-PREPOST, these are the average values. 
21.11  Strain Rate Effects in Material Models 
In  a  constitutive  modeling  context,  the  term  rate  effects  is  used  to  indicate  that  the 
material response depends on the (time) rate of a certain quantity, here called 𝑒 for the 
sake  of  generality.    This  quantity  is  usually  some  kind  of  strain  measure,  and  an 
example is when the stress depends on the rate of strain.  In explicit simulations, high 
frequency  strain  content  yields  a  very  noisy  strain  rate  and  calls  for  some  kind  of 
smoothing  before  being  used  in  the  stress  calculations.    This  section  presents  three  of 
the  common  ways  to  do  this  averaging  and  that  are  used  frequently  in  the  material 
models. 
21.11.1  Running N-average option 
One  option  is  to  do  a running  average of  current  and  previous  strain  rates.    With  this 
option the rate 𝑒 ̇ of a quantity 𝑒 is averaged according to the following algorithm
LS-DYNA Theory Manual 
Stress Update Overview 
̇ = unfiltered rate (raw data)
𝑒 ̃
𝑒 ̃
𝑒 ̇𝑛 =
̇+ ∑
𝑛−1
𝑖=𝑛−𝑁+1
𝑒 ̇𝑖
𝑒 ̇ = 𝑒 ̇𝑛 = rate used in material routine 
(21.1)
(21.2)
(21.3)
In  these  equations,  the  subscript  denotes  stored  history  variables  necessary  for 
computing  the  running  average  strain  rates  and  n  denotes  the  current  cycle  number.  
This requires storage of 𝑁 − 1 history variables, for most materials 𝑁 = 12. 
21.11.2  Last N-average option 
The second option is to compute the rate as  the average of the last 𝑁 computed rates.  
Here the rate is evaluated according to 
𝑒 ̃
̇ = unfiltered rate (raw data)
̇ 
𝑒 ̇𝑛 = 𝑒 ̃
𝑒 ̇ =
∑
𝑖=𝑛−𝑁+1
𝑒 ̇𝑖
= rate used in material routine 
(21.4)
(21.5)
(21.6)
As  for  the  running  average  option,  the  subscript  denotes  stored  history  variables 
necessary  for  computing  the  running  average  strain  rates  and  n  is  the  cycle  number.  
This also requires storage of 𝑁 − 1 history variables, for most materials 𝑁 = 12. 
21.11.3  Averaging over a fixed amount of time 𝑻 
This  option  was  introduced  in  an  attempt  to  suppress  the  time  step  dependence  as 
much as possible.  With this option we use 𝑁 history variables to store the approximate 
values of the quantity of interest from the time 𝑡𝑛 − 𝑇 to current time 𝑡𝑛. That is, we set 
𝑒𝑛−𝑖 = 𝑒𝑛 (𝑡𝑛 −
𝑖𝑇
𝑁 − 1
) , 𝑖 = 0, … , 𝑁 − 1
(21.7)
Here 𝑒𝑛(𝑡) is an approximate function of the function of interest, 𝑒(𝑡), and will be given 
more specifically below.  Assuming 𝑒𝑛(𝑡) is known, the rate used in the material routine 
in cycle 𝑛 is simply 
𝑒 ̇ =
𝑒𝑛 − 𝑒𝑛−𝑁+1
= rate used in material routine
(21.8)
For the update of history variables we assume that the 𝑁 points in (21.7) together with 
the newly calculated quantity (raw data) at 𝑡𝑛+1 = 𝑡 + ∆𝑡, 
(21.9)
completely define the function 𝑒𝑛(𝑡) from time 𝑡𝑛 − 𝑇 to time 𝑡𝑛+1 by linear interpolation 
between each  control point.  That is, the  function 𝑒𝑛(𝑡) is extended to time  𝑡𝑛+1 by the 
new value, 
𝑒𝑛+1 = 𝑒(𝑡𝑛+1),
𝑒𝑛(𝑡𝑛+1) = 𝑒𝑛+1.
(21.10)
Stress Update Overview 
LS-DYNA Theory Manual 
This function is illustrated in the figure below by the dashed line and red control points.  
The updated set of history variables are 
𝑒𝑛+1−𝑖 = 𝑒𝑛 (𝑡𝑛+1 −
𝑖𝑇
𝑁 − 1
) , 𝑖 = 0, … , 𝑁 − 1,
(21.11)
and  these  updated  points  define  a  new  approximate  function  𝑒𝑛+1(𝑡),  again  by  linear 
interpolation  between  the  control  points.    In  Figure  21.1,  the  updated  function  is 
illustrated by the solid line and blue control points, note that the last point is in fact both 
red and blue since 𝑒𝑛(𝑡𝑛+1) = 𝑒𝑛+1(𝑡𝑛+1) = 𝑒𝑛+1. In sum, the function used for calculated 
the effective rate is completely redefined between steps. 
For a time step ∆𝑡 that is greater than or approximately equal to 𝑇/(𝑁 − 1), this option 
is more or less exactly the average rate from 𝑡 − 𝑇 to 𝑡. For smaller time steps (which is 
usually  the  case  in  explicit  analysis)  the  previous  values  are  in  practice  smoothed  out 
since  only  𝑁  variables  are  available  for  storing  this  time  history.    That  is,  the  high 
frequency content of the history is lost and this could be an interesting alternative to the 
previous two options that are otherwise commonly used for these types of situations. 
𝑒 
Control points and function 𝑒𝑛(𝑡) 
Control points and function 𝑒𝑛+1(𝑡) 
𝑒𝑛+1 = 𝑒(𝑡𝑛+1) 
𝑡𝑛
𝑡𝑛+1
𝑡𝑛 − 𝑇 
Figure 21.1.  Illustration of control point update for 𝑁 = 4 
21.12  Algorithmic Consistent Tangent Modulus for Plasticity 
For  materials  used  in  implicit  analysis,  the  tangent  modulus  is  needed  for  global 
assembly  of  the  stiffness  matrix.    In  particular,  the  softening  effect  in  elastic-plastic 
materials must be predicted when in a plastic state.  The following is a derivation of the 
tangent  modulus  that  is  consistent  with  the  algorithmic  stress  update,  meaning  that  it 
provides  the  exact  variation  of  the  stress  with  respect  to  the  rate  of  deformation.    We 
restrict ourselves to the plane stress update, as the full 3D situation is less complicated.
LS-DYNA Theory Manual 
Stress Update Overview 
As  a  prerequisite,  the  algorithmic  stress  update  must  be  established  mathematically.  
For this, and the rest of this section, we introduce the variables 
Δ𝝈 −  stress increment, excluding through thickness stress ∆𝜎3 
∆𝜀3 − through thickness strain increment 
∆𝜀𝑝 − plastic strain increment 
∆𝜶 − back stress increment, full tensor 
to be sought, the parameters 
𝑪 − 3𝐷 elastic tensor 
Δ𝜺 −  strain increment, excluding through thickness strain ∆𝜀3 
𝑷 − projection from 3D to plane stress space 
𝒑𝑇 − projection from 3D to out of plane space 
that are given, and the functions 
𝑓 (𝑷𝑇Δ𝝈 − Δ𝜶, ∆𝜀𝑝) − yield function 
𝑔(𝑷𝑇Δ𝝈 − Δ𝜶, ∆𝜀𝑝) − plastic flow function 
ℎ(𝑷𝑇Δ𝝈 − Δ𝜶, ∆𝜀𝑝) − back stress potential 
that define the plasticity.  This theory thus incorporates full anisotropy as well as non-
associative plasticity.  The stress update can be summarized by the combination of four 
equations; the stress update 
Δ𝝈 = 𝑷𝑪
⎜⎛𝑷𝑇∆𝜺 + 𝒑∆𝜀3 − {
⎝
}
𝜕𝑔
𝜕𝝈
∆𝜀𝑝
⎟⎞, 
⎠
(21.12)
the yield condition 
𝑓 = 𝜎(𝑷𝑇(𝝈0 + Δ𝝈) − (𝜶0 + Δ𝜶)) − 𝜎𝑌(𝜀0 + ∆𝜀𝑝) = 0, 
(21.13)
the evolution of back stress 
Δ𝜶 = {
}
𝜕ℎ
𝜕𝝈
∆𝜀𝑝, 
and the plane stress condition 
∆𝜎3 = 𝒑𝑇𝑪
⎜⎛𝑷𝑇∆𝜺 + 𝒑∆𝜀3 − {
⎝
}
∆𝜀𝑝
𝜕𝑔
𝜕𝝈
⎟⎞ = 0. 
⎠
(21.14)
(21.15)
The expression for 𝑓  in (21.13) is in terms of effective stress 𝜎 equals the yield stress 𝜎𝑌, but 
the theory is not restricted to this setting.  It is assumed that the stress 𝝈0, back stress 𝜶0
Stress Update Overview 
LS-DYNA Theory Manual 
and the plastic strain 𝜀0 in the previous step fulfils the corresponding conditions (21.12), 
(21.13), (21.14) and (21.15) with respect to the state at that time, possibly with inequality 
in (21.13). 
Taking the variation of these four equations results in  
δΔ𝝈 = 𝑷𝑪
}
δ∆𝜀𝑝 −
𝜕𝑔
𝜕𝝈
𝜕2𝑔
𝜕𝝈2 (𝑷𝑇δΔ𝝈 − δΔ𝜶)∆𝜀𝑝
⎜⎛𝑷𝑇δ∆𝜺 + 𝒑δ∆𝜀3 − {
⎝
−
𝜕2𝑔
𝜕𝝈𝜕𝜀𝑝
δΔ𝜀𝑝∆𝜀𝑝
⎟⎞, 
⎠
(𝑷𝑇δΔ𝝈 − δΔ𝜶) +
𝜕𝑓
𝜕𝜀𝑝
δΔ𝜀𝑝 = 0, 
𝜕𝑓
𝜕𝝈
δΔ𝜶 = {
𝜕ℎ
𝜕𝝈
}
δ∆𝜀𝑝 +
𝜕2ℎ
𝜕𝝈2 (𝑷𝑇δΔ𝝈 − δΔ𝜶)∆𝜀𝑝 +
𝜕ℎ
𝜕𝝈𝜕𝜀𝑝
δ∆𝜀𝑝∆𝜀𝑝, 
(21.16)
(21.17)
(21.18)
𝒑𝑇𝑪
⎜⎛𝑷𝑇δ∆𝜺 + 𝒑δ∆𝜀3 − {
⎝
= 0. 
}
δ∆𝜀𝑝 −
𝜕𝑔
𝜕𝝈
𝜕2𝑔
𝜕𝝈2 (𝑷𝑇δΔ𝝈 − δΔ𝜶)∆𝜀𝑝 −
𝜕2𝑔
𝜕𝝈𝜕𝜀𝑝
δΔ𝜀𝑝∆𝜀𝑝
⎟⎞
⎠
(21.19)
Solving (21.16) and (21.18) for 𝑷𝑇δΔ𝝈 − δΔ𝜶 results in 
𝑷𝑇δΔ𝝈 − δΔ𝜶 = 𝑨−1𝑷𝑇𝑷𝑪𝑷𝑇δ∆𝜺 + 𝑨−1𝑷𝑇𝑷𝑪𝒑δ∆𝜀3 − 𝑨−1𝑭δ∆𝜀𝑝 
(21.20)
where  
𝑨 = 𝑰 + 𝑷𝑇𝑷𝑪
𝜕2ℎ
𝜕𝝈2 ∆𝜀𝑝 
}
+
𝜕𝑔
𝜕𝝈
𝜕2𝑔
𝜕𝝈2 ∆𝜀𝑝 +
𝜕2𝑔
𝜕𝝈𝜕𝜀𝑝
𝜕2ℎ
𝜕𝝈𝜕𝜀𝑝
𝑭 = 𝑷𝑇𝑷𝑪𝑮 + 𝑯.
𝜕ℎ
𝜕𝝈
}
+
𝑮 = {
𝑯 = {
∆𝜀𝑝 
∆𝜀𝑝 
(21.21)
Inserting (21.20) into (21.17) and (21.19) results in a system of equations 
𝒑𝑇𝑬𝑪𝒑
𝑨−1𝑷𝑇𝑷𝑪𝒑
⎜⎜⎜⎜⎛
⎝
−
𝜕𝑓
𝜕𝝈
𝒑𝑇𝑳
𝑨−1𝑭 −
𝜕𝑓
𝜕𝝈
⎟⎟⎟⎟⎞
𝜕𝑓
𝜕𝜀𝑝⎠
(
δ∆𝜀3
δ∆𝜀𝑝
) =
−𝒑𝑇𝑬
⎟⎟⎟⎞
𝑨−1𝑷𝑇𝑷⎠
⎜⎜⎜⎛
⎝
𝜕𝑓
𝜕𝝈
𝑪𝑷𝑇δ∆𝜺. 
(21.22)
where
LS-DYNA Theory Manual 
Stress Update Overview 
Solving (21.22) results in 
and 
𝜕2𝑔
𝜕𝝈2 𝑨−1𝑷𝑇𝑷∆𝜀𝑝 
𝑬 = 𝑰 − 𝑪
𝜕2𝑔
𝜕𝝈2 𝑨−1𝑭∆𝜀𝑝 − 𝑮). 
𝑳 = 𝑪 (
δ∆𝜀3 = 𝒂3
𝑇𝑩𝑪𝑷𝑇δ∆𝜺
δ∆𝜀𝑝 = 𝒂𝑝
𝑇𝑩𝑪𝑷𝑇δ∆𝜺 
(21.23)
(21.24)
(21.25)
𝑇  and  𝒂𝑝
𝑇  are  rows  in  the  inverse  of  the  system  matrix  in (21.22)  and  𝑩  can  be 
where 𝒂3
identified on the right-hand side of the same equation.  Inserting (21.24) and (21.25) into 
(21.20) results in 
δΔ𝝈 = 𝑷(𝑬 + 𝑬𝑪𝒑𝒂3
𝑇𝑩 + 𝑳𝒂𝑝
𝑇𝑩)𝑪𝑷𝑇δ∆𝜺 
from which the consistent tangent matrix can be identified as 
𝑫 = 𝑷(𝑬 + 𝑬𝑪𝒑𝒂3
𝑇𝑩 + 𝑳𝒂𝑝
𝑇𝑩)𝑪𝑷𝑇. 
(21.26)
(21.27)
Even  though  the  involved  expressions  seem  complicated,  many  expressions  are 
repeated, and they simplify quite a bit when considering special cases.  As an example, 
consider  isotropic  von  Mises  plasticity  with  linear  hardening  and  back  stress  (mixed 
formulation) for which we have 
𝑓 = 𝑔 = 𝜎 − 𝜎𝑌 − 𝛽𝐻𝜀𝑝
ℎ =
(1 − 𝛽)𝐻𝑓  
(21.28)
where  𝜎 = √3
Then 
2 𝒔𝑇𝒔  and  𝒔  is  the  deviatoric  stress,  including  subtraction  of  back  stress  𝜶. 
𝜕𝑓
𝜕𝝈
𝜕ℎ
𝜕𝝈
=
=
=
𝜕𝑔
𝜕𝝈
2𝜎
(1 − 𝛽)𝐻
𝒔𝑇 
𝒔𝑇 
and 
(𝑰𝑑𝑒𝑣 −
𝜕2𝑔
𝜕𝝈2 =
2𝜎
(1 − 𝛽)𝐻
𝜕2ℎ
𝜕𝝈2 =
2𝜎 2 𝒔𝒔𝑇) 
2𝜎 2 𝒔𝒔𝑇) 
(𝑰𝑑𝑒𝑣 −
(21.29)
(21.30)
Stress Update Overview 
LS-DYNA Theory Manual 
If the elastic matrix 𝑪 is isotropic, then we have 
and 
𝜕𝑓
𝜕𝝈
𝑪 =
3𝐺
𝒔𝑇 
𝜕2𝑔
𝜕𝝈2 =
3𝐺
(𝑰𝑑𝑒𝑣 −
2𝜎 2 𝒔𝒔𝑇) 
(21.31)
(21.32)
with  𝐺  being  the  shear  modulus,  resulting  in  an  𝑨  matrix  that  is  invertible  on  closed 
form.  We also have 
𝜕2𝑔
𝜕𝝈𝜕𝜀𝑝
=
𝜕2ℎ
𝜕𝝈𝜕𝜀𝑝
= 𝟎. 
(21.33)
In  3D  constitutive  laws,  𝑷 = 𝑰  and  𝒑 = 𝟎,  so  the  system  (21.22)  reduces  to  a  scalar 
𝑇 = 𝟎  in  (21.27),  and  so  on,  so  the  implementation  is  very  much 
equation  with  𝒂3
tractable.
LS-DYNA Theory Manual 
Material Models 
22    
Material Models 
LS-DYNA  accepts  a  wide  range  of  material  and  equation  of  state  models,  each 
with  a  unique  number  of  history  variables.    Approximately  150  material  models  are 
implemented, and space has been allotted for up to 10 user-specified models. 
Elastic  
Orthotropic Elastic 
Kinematic/Isotropic Elastic-Plastic 
Thermo-Elastic-Plastic 
Soil and Crushable/Non-crushable Foam 
Viscoelastic 
Blatz - Ko Rubber 
High Explosive Burn 
Null Hydrodynamics 
Isotropic-Elastic-Plastic-Hydrodynamic 
Temperature Dependent, Elastoplastic, Hydrodynamic 
Isotropic-Elastic-Plastic 
Elastic-Plastic with Failure Model 
Soil and Crushable Foam with Failure Model 
Johnson/Cook Strain and Temperature Sensitive Plasticity 
Pseudo TENSOR Concrete/Geological Model 
Isotropic Elastic-Plastic Oriented Crack Model 
Power Law Isotropic Plasticity 
Strain Rate Dependent Isotropic Plasticity 
Rigid 
Thermal Orthotropic Elastic 
Composite Damage Model 
Thermal Orthotropic Elastic with 12 Curves 
Piecewise Linear Isotropic Plasticity 
Inviscid Two Invariant Geologic Cap Model 
1  
2  
3  
4  
5  
6  
7  
8  
9  
10  
11  
12  
13  
14  
15  
16  
17  
18  
19  
20  
21  
22  
23  
24  
25  
26   Metallic Honeycomb
Material Models 
LS-DYNA Theory Manual 
Planar Anisotropic Plasticity Model 
Strain Rate Dependent Plasticity with Size Dependent Failure 
Temperature and Rate Dependent Plasticity 
Sandia’s Damage Model 
Low Density Closed Cell Polyurethane Foam 
Compressible Mooney-Rivlin Rubber 
Resultant Plasticity 
Force Limited Resultant Formulation 
Closed-Form Update Shell Plasticity 
Slightly Compressible Rubber Model 
Laminated Glass Model 
Barlat’s Anisotropic Plasticity Model 
Fabric 
Kinematic/Isotropic Elastic-Plastic Green-Naghdi Rate 
Barlat’s 3-Parameter Plasticity Model 
Transversely Anisotropic Elastic-Plastic 
Blatz-Ko Compressible Foam 
Transversely Anisotropic Elastic-Plastic with FLD 
27  
28  
29  
30  
31  
32  
33  
34  
35  
36  
37  
38  
39  
40   Nonlinear Elastic Orthotropic Material 
41-50  User Defined Material Models 
42  
48 
51  
52  
53  
54-55   Composite Damage Model 
57 
Low Density Urethane Foam 
58 
Laminated Composite Fabric 
59 
Composite Failure 
Elastic with Viscosity 
60  
61   Maxwell/Kelvin Viscoelastic 
62  
63  
64  
65   Modified Zerilli/Armstrong 
66  
67   Nonlinear Stiffness/Viscous 3D Discrete Beam 
68   Nonlinear Plastic/Linear Viscous 3D Discrete Beam 
69  
Side Impact Dummy Damper, SID Damper 
70   Hydraulic/Gas Damper 
71  
72  
73 
74 
75 
76   General Viscoelastic 
77   Hyperviscoelastic Rubber 
78  
Soil/Concrete 
79   Hysteretic Soil 
80  
Cable 
Concrete Damage Model 
Low Density Viscoelastic Foam 
Elastic Spring for the Discrete Beam 
Bilkhu/Dubois Foam Model 
Viscous Foam 
Isotropic Crushable Foam 
Strain Rate Sensitive Power-Law Plasticity 
Linear Stiffness/Linear Viscous 3D Discrete Beam 
Ramberg-Osgood Plasticity
LS-DYNA Theory Manual 
Material Models 
Plastic with Damage 
Isotropic Elastic-Plastic with Anisotropic Damage 
Fu-Chang’s Foam with Rate Effects 
Plasticity Polymer 
81  
82 
83 
84-85  Winfrith Concrete 
84  Winfrith Concrete Reinforcement 
86   Orthotropic-Viscoelastic 
87  
Cellular Rubber 
88  MTS Model 
89 
90   Acoustic 
Soft Tissue 
91 
Elastic 6DOF Spring Discrete Beam 
93 
Inelastic Spring Discrete Beam 
94 
Inelastic 6DOF Spring Discrete Beam 
95 
96 
Brittle Damage Model 
97   General Joint Discrete Beam 
100   Spot weld 
101  GE Thermoplastics 
102  Hyperbolic Sin 
103  Anisotropic Viscoplastic 
104  Damage 1 
105  Damage 2 
106 
110  
111  
112 
113 
114 
115   Elastic Creep Model  
116   Composite Lay-Up Model 
117-118 
119  General Spring and Damper Model 
120   Gurson Dilational-Plastic Model 
120  Gurson Model with Rc-Dc 
121  Generalized Nonlinear 1DOF Discrete Beam 
122  Hill 3RC 
123  Modified Piecewise Linear Plasticity 
Tension-Compression Plasticity 
124 
126   Metallic Honeycomb 
127  Arruda-Boyce rubber 
128  Anisotropic heart tissue 
129 
Lung tissue 
130   Special Orthotropic 
131 
132  Orthotropic Smeared Crack 
Elastic Viscoplastic Thermal 
Johnson-Holmquist Ceramic Model 
Johnson-Holmquist Concrete Model 
Finite Elastic Strain Plasticity 
Transformation Induced Plasticity 
Layered Linear Plasticity 
Isotropic Smeared Crack 
Composite Matrix
Material Models 
LS-DYNA Theory Manual 
EMMI 
Barlat  YLD2000 
Composite MSC 
Pitzer Crushable Foam 
Schwer Murray Cap Model 
1DOF Generalized Spring 
FHWA Soil Model 
133 
134   Viscoelastic Fabric 
139  Modified Force Limited 
140  Vacuum 
141  Rate Sensitive Polymer 
142   Transversely Anisotropic Crushable Foam 
143  Wood Model 
144 
145 
146 
147 
148  Gas Mixture  
150  CFD 
151 
154  Deshpande-Fleck Foam 
156  Muscle 
158  Rate Sensitive Composite Fabric 
159  Continuous Surface Cap Model 
161-162 
163  Modified Crushable Foam 
164   Brain Linear Viscoelastic 
166  Moment Curvature Beam 
169  Arup Adhesive 
170  Resultant Anisotropic 
175  Viscoelastic Maxwell 
176  Quasilinear Viscoelastic 
177  Hill Foam 
178  Viscoelastic Hill Foam 
179   Low Density Synthetic Foam 
181 
183 
184  Cohesive Elastic 
185  Cohesive TH 
191 
Seismic Beam 
192   Soil Brick 
193  Drucker Prager 
194  RC Shear Wall 
195  Concrete Beam 
196  General Spring Discrete Beam 
197 
198 
Simplified Rubber/Foam 
Simplified Rubber with Damage 
Seismic Isolator 
Jointed Rock
LS-DYNA Theory Manual 
Material Models 
In  the  table  below,  a  list  of  the  available  material  models  and  the  applicable  element 
types  are  given.    Some  materials  include  strain  rate  sensitivity,  failure,  equations  of 
state, and thermal effects and this is also noted.  General applicability of the materials to 
certain kinds of behavior is suggested in the last column. 
Notes: 
 Gn  Gen-
eral 
 Cm  Com-
posites 
 Cr  Ceram-
ics 
 Fl 
Fluids 
 Fm  Foam 
 Gl  Glass 
 Hy  Hydro-
dyn 
 Mt  Metal 
 Pl 
Plastic 
 Rb  Rubber
 Sl
Soil/C
onc 
ff
-
-
-
ff
Y Y Y Y  
Y   Y Y  
- 
  Gn, Fl 
  Cm, Mt 
Y Y Y Y Y Y  
Y Y Y Y  
Y  
Y Y Y   Y  
Y   Y  
  Cm, Mt, Pl 
  Y  Mt, Pl 
Fm, Sl 
  Rb 
  Rb, 
Polyurethane 
Material Title 
(Anisotropic 
Elastic 
Orthotropic  Elastic 
solids) 
Plastic Kinematic/Isotropic 
Elastic Plastic Thermal 
Soil and Foam 
Linear Viscoelastic 
Blatz-Ko Rubber 
Temp. 
High Explosive Burn 
Null Material 
Elastic Plastic Hydro(dynamic) 
Steinberg: 
Elastoplastic  
Isotropic  Elastic Plastic 
Isotropic Elastic Plastic with Failure 
Soil and Foam with Failure 
Johnson/Cook Plasticity Model 
Pseudo TENSOR Geological Model 
Dependent 
Y  
Y  
Y  
Y  
  Y    Hy 
  Y Y  Y  Fl, Hy 
  Y Y    Hy, Mt 
  Y Y Y  Y  Hy, Mt 
  Mt 
  Mt 
Y   Y Y  
  Y  
Y  
Fm, Sl 
  Y  
Y  
Y   Y   Y Y Y  Y  Hy, Mt 
  Y Y Y   
Y  
Sl 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
11 
12 
13 
14 
15 
16
Material Models 
LS-DYNA Theory Manual 
  (Elastoplastic  with 
17  Oriented  Crack 
Fracture) 
Power Law Plasticity  (Isotropic) 
Strain Rate Dependent Plasticity 
18 
19 
20  Rigid 
Y  
  Y Y    Hy, Mt, Pl 
Y Y Y Y Y  
Y   Y Y Y Y  
Y Y Y Y  
  Mt, Pl 
  Mt, Pl 
Notes: 
 Gn  Gen-
eral 
 Cm  Com-
posites 
 Cr  Ce-
ramics 
 Fl 
Fluids 
 Fm  Foam 
 Gl  Glass 
 Hy
Hydro
-dyn 
 Mt  Metal 
 Pl 
Plastic 
 Rb  Rubber
 Sl
Soil/C
onc 
Material Title 
ff
-
-
-
ff
Temperature Dependent Orthotropic 
Piecewise Linear Plasticity  (Isotropic) 
Inviscid Two Invariant Geologic Cap 
21  Orthotropic Thermal (Elastic) 
22  Composite Damage 
23 
24 
25 
26  Honeycomb 
27  Mooney-Rivlin Rubber 
28  Resultant Plasticity 
29 
Force Limited Resultant Formulation 
30  Closed Form Update Shell Plasticity 
Slightly Compressible Rubber 
31 
Laminated Glass (Composite) 
32 
Barlat Anisotropic Plasticity 
33 
Fabric 
34 
Plastic Green-Naghdi Rate 
35 
3-Parameter Barlat Plasticity 
36 
Transversely Anisotropic Elastic Plastic 
37 
Y   Y Y  
Y   Y Y   Y  
Y   Y Y  
Y Y Y Y Y Y  
Y  
Y  
Y   Y  
  Y Y  
  Y  
  Y Y  
  Y  Gn 
  Cm 
  Y  Cm 
  Mt, Pl 
Sl 
  Cm, Fm, Sl 
  Rb 
  Mt 
  Y Y  
Y  
  Y Y   Y  
Y   Y Y  
  Y  
Y  
  Y  
  Y  
  Y Y  
  Mt 
  Rb 
  Cm, Gl 
  Cr, Mt 
  Mt 
  Mt 
  Mt
LS-DYNA Theory Manual 
Material Models 
Blatz-Ko Foam 
FLD Transversely Anisotropic 
38 
39 
40  Nonlinear Orthotropic 
Y   Y  
Fm, Pl 
  Y Y  
  Y  
  Mt 
  Y   Y  Cm 
41-
50
42 
User Defined Materials 
Y Y Y Y Y Y Y  Y  Gn 
Planar Anisotropic Plasticity Model 
Notes: 
 Gn  Gen-
eral 
 Cm  Com-
posites 
 Cr  Ce-
ramics 
 Fl 
Fluids 
 Fm  Foam 
 Gl  Glass 
 Hy
Hydro
-dyn 
 Mt  Metal 
 Pl 
Plastic 
 Rb  Rubber
 Sl
Soil/C
onc 
Material Title 
ff
-
-
-
ff
51 
Bamman 
Plasticity) 
52 
Bamman Damage 
53  Closed  Cell  Foam 
Polyurethane) 
(Temp/Rate  Dependent 
Y   Y Y Y  
  Y  Gn 
(Low  Density 
Y   Y Y Y Y   Y  Mt 
Fm 
Y  
54  Composite  Damage  with  Change 
  Y  
  Y  
  Cm 
Failure 
55  Composite  Damage  with  Tsai-Wu 
  Y  
  Y  
  Cm 
Failure 
56 
Low Density Urethane Foam 
57 
58 
Laminated Composite Fabric 
59  Composite Failure  (Plasticity Based) 
Elastic with Viscosity  (Viscous Glass) 
60 
61  Kelvin-Maxwell Viscoelastic 
62  Viscous Foam  (Crash Dummy Foam) 
63 
Isotropic Crushable Foam 
Y  
  Y Y  
Fm 
  Y  
  Cm, Cr 
  Y  
Y   Y  
Y   Y   Y  
  Y  
Y  
  Y  
Y  
  Y  
Y  
  Y  Gl 
Fm 
Fm 
Fm
Material Models 
LS-DYNA Theory Manual 
(Rate/Temp 
64  Rate Sensitive Powerlaw Plasticity 
65  Zerilli-Armstrong 
Plasticity) 
Linear Elastic Discrete Beam 
66 
67  Nonlinear Elastic Discrete Beam 
68  Nonlinear Plastic Discrete Beam 
69 
SID Damper Discrete Beam 
70  Hydraulic Gas Damper Discrete Beam 
71  Cable Discrete Beam (Elastic) 
72  Concrete Damage 
  Mt 
Y   Y Y Y  
Y   Y   Y   Y  Y  Mt 
  Y  
  Y  
  Y  
  Y  
  Y  
  Y  
Y  
  Y  
  Y  
  Y Y  
  Y  
  Y  
  Y Y Y   
Sl 
Notes: 
 Gn  General 
 Cm  Compo-
sites 
 Cr  Ceramics
Fluids 
 Fl 
 Fm  Foam 
 Gl  Glass 
 Hy  Hydro-
dyn 
 Mt  Metal 
Plastic 
 Pl 
 Rb  Rubber 
 Sl
Soil/Con
c 
Material Title 
ff
-
-
-
ff
73  Low Density Viscous Foam 
Y  
  Y Y  
Fm 
74  Elastic Spring for the Discrete Beam 
75  Bilkhu/Dubois Foam (Isotropic) 
Y  
76  General Viscoelastic (Maxwell Model) Y  
77  Hyperelastic and Ogden Rubber 
78 
Soil Concrete 
Y  
Y  
  Y  
  Y  
  Y  
79  Hysteretic  Soil 
(Elasto-Perfectly 
Y  
  Y  
Fm 
  Rb 
  Rb 
Sl 
Sl 
Plastic) 
80  Ramberg Osgood Plasticity 
81  Plasticity  with  Damage 
(Elasto-
Y Y Y Y Y Y  
  Mt, Pl 
82 
Plastic) 
Isotropic 
Anisotropic Damage 
Elastic-Plastic 
with
LS-DYNA Theory Manual 
Material Models 
83 
Fu Chang Foam 
84  Winfrith Concrete Reinforcement 
Y  
Y  
  Y Y  
Fm 
85 
86  Orthotropic Viscoelastic 
87  Cellular Rubber 
88  MTS 
89  Plasticity Polymer 
90  Acoustic 
91 
Soft Tissue 
  Y   Y  
Y  
  Y  
  Rb 
  Rb 
Y   Y   Y   Y   Mt 
  Y  
Y  
Y   Y  
Fl 
93  Elastic 6DOF Spring Discrete Beam 
  Y  
94 
Inelastic Spring Discrete Beam 
  Y  
Notes: 
 Gn  General 
 Cm  Compo-
sites 
 Cr  Ceram-
ics 
Fluids 
 Fl 
 Fm  Foam 
 Gl  Glass 
 Hy  Hydro-
dyn 
 Mt  Metal 
Plastic 
 Pl 
 Rb  Rubber 
 Sl
Soil/Co
nc 
ff
-
-
-
ff
Material Title 
Inelastic 6DOF Spring Discrete Beam 
  Y  
Brittle Damage 
Y  
  Y Y  
95 
96 
97  General Joint Discrete Beam 
  Y  
98 
99 
Simplified Johnson Cook 
Y Y Y Y  
Simplified  Johnson  Cook  Orthotropic 
Damage 
100  Spotweld 
LS-DYNA Draft
Material Models 
LS-DYNA Theory Manual 
101  GEPLASTIC Strate2000a 
102 
Inv Hyperbolic Sin 
103  Anisotropic Viscoplastic 
104  Damage 1 
105  Damage 2 
106  Elastic Viscoplastic Thermal 
  Y  
Y  
Y   Y  
Y   Y  
Y   Y  
Y   Y  
  Y 
107 
108 
109 
110 
Johnson Holmquist Ceramics 
111 
Johnson Holmquist Concrete 
112  Finite Elastic Strain Plasticity 
Y  
Y  
Y  
113  TRIP 
  Y Y  
  Y  Mt 
114  Layered Linear Plasticity 
  Y Y  
115  Unified Creep 
Y  
Notes: 
 Gn  General 
 Cm  Compo-
sites 
 Cr  Ceram-
ics 
 Fl 
Fluids 
 Fm  Foam 
 Gl  Glass 
 Hy  Hydro-
dyn 
 Mt  Metal 
Plastic 
 Pl 
 Rb  Rubber 
 Sl
Soil/Co
nc 
Material Title 
116  Composite Layup 
117  Composite Matrix 
118  Composite Direct 
ff
-
-
-
ff
  Y  
  Y  
  Y
LS-DYNA Theory Manual 
Material Models 
119  General  Nonlinear  6DOF  Discrete 
  Y  
  Y Y  
Beam 
120  Gurson 
  Y  
121  Generalized  Nonlinear  1DOF  Discrete 
  Y  
Beam 
122  Hill 3RC 
123  Modified Piecewise Linear Plasticity 
  Y Y  
124  Plasticity Compression Tension 
126  Modified Honeycomb 
127  Arruda Boyce Rubber 
128  Heart Tissue 
129  Lung Tissue 
Y  
Y  
Y  
Y  
Y  
130  Special Orthotropic 
  Y  
131 
Isotropic Smeared Crack 
132  Orthotropic Smeared Crack 
133  Barlat YLD2000 
Y  
Y  
  Y  
  Mt, Cm 
  Y  
  Mt, Cm 
139  Modified Force Limited 
  Y  
140  Vacuum 
141  Rate Sensitive Polymer 
Notes: 
 Gn  General 
 Cm  Compo-
sites 
 Cr  Ceramics
 Fl 
Fluids 
 Fm  Foam 
 Gl  Glass 
 Hy  Hydro-
dyn 
 Mt  Metal 
 Pl 
Plastic 
 Rb  Rubber 
 Sl
Soil/Con
c 
Material Title 
ff
-
-
-
ff
Material Models 
LS-DYNA Theory Manual 
142  Transversely  Anisotropic  Crushable 
Foam 
143  Wood 
144  Pitzer Crushable Foam 
145  Schwer Murray Cap Model 
146  1DOF Generalized Spring 
147  FHWA Soil 
147  FHWA Soil Nebraska 
148  Gas Mixture 
150  CFD 
151  EMMI 
154  Deshpande Fleck Foam 
Y  
  Y Y Y   Y  Mt 
156  Muscle 
  Y  
  Y  
158  Rate Sensitive Composite Fabric 
  Y Y Y Y  
  Cm 
159  CSMC 
161  Composite MSC 
163  Modified Crushable Foam 
164  Brain Linear Viscoelastic 
  Y Y Y  
Sl 
Y  
Y  
166  Moment Curvature Beam 
  Y  
169  Arup Adhesive 
170  Resultant Anisotropic 
175  Viscoelastic Thermal 
176  Quasilinear Viscoelastic 
Y  
  Y   Y  
  Y Y  
Pb 
Pl 
Y   Y Y Y  
  Y  Rb
LS-DYNA Theory Manual 
Material Models 
Notes: 
 Gn  General 
 Cm  Compo-
sites 
 Cr  Ceramics
 Fl 
Fluids 
 Fm  Foam 
 Gl  Glass 
 Hy  Hydro-
dyn 
 Mt  Metal 
 Pl 
Plastic 
 Rb  Rubber 
 Sl
Soil/Con
c 
ff
-
-
-
ff
Material Title 
177  Hill Foam 
178  Viscoelastic Hill Foam 
179  Low Density Synthetic Foam 
181  Simplified Rubber 
183  Simplified Rubber with Damage 
Y   Y Y Y Y  
  Rb 
184  Cohesive Elastic 
185  Cohesive TH 
191  Seismic Beam 
192  Soil Brick 
193  Drucker Prager 
194  RC Shear Wall 
195  Concrete Beam 
196  General Spring Discrete Beam 
197  Seismic Isolator  
198 
Jointed Rock 
Spring Elastic (Linear) 
Y  
Y  
  Y  
Y  
Y  
  Y  
  Y  
  Y  
  Y  
Y  
  Y  
  Y  
  Cm, Mt 
  Y  
  Cm, Mt 
  Y  
  Mt 
  Y  
Damper Viscous (Linear) 
  Y  
  Y  
Spring Elastoplastic (Isotropic) 
  Y  
DS
1 
DS
2 
DS
Material Models 
LS-DYNA Theory Manual 
Spring Nonlinear Elastic 
  Y  
  Y  
Damper Nonlinear Elastic 
  Y  
  Y  
Spring General Nonlinear 
  Y  
DS
4 
DS
5 
DS
6 
Material Title 
Spring  Maxwell  (Three  Parameter 
Viscoelastic) 
Spring 
Compression) 
Spring Trilinear Degrading 
(Tension 
Inelastic 
or 
Spring Squat Shearwall 
Spring Muscle 
DS
7 
DS
8 
DS
13 
DS
14 
DS
15 
SB1  Seatbelt 
Notes: 
 Gn  General 
 Cm  Compo-
sites 
 Cr  Ceramics
 Fl 
Fluids 
 Fm  Foam 
 Gl  Glass 
 Hy  Hydro-
dyn 
 Mt  Metal 
 Pl 
Plastic 
 Rb  Rubber 
 Sl
Soil/Con
c 
ff
-
-
-
ff
  Y  
  Y  
  Y  
T01  Thermal Isotropic 
T02  Thermal Orthotropic 
Y   Y  
Y   Y  
T03  Thermal 
Isotropic 
(Temp.  
Y   Y  
Dependent) 
T04  Thermal 
Orthotropic 
(Temp.  
Y   Y  
Dependent) 
T05  Thermal Isotropic (Phase Change) 
Y   Y  
  Y 
  Y 
  Y 
  Y 
  Y
LS-DYNA Theory Manual 
Material Models 
T06  Thermal  Isotropic  (Temp  Dep-Load 
Y   Y  
Curve) 
T11  Thermal User Defined 
Y   Y  
  Y 
  Y
Material Models 
LS-DYNA Theory Manual 
22.1  Material Model 1:  Elastic 
In this elastic material we compute the co-rotational rate of the deviatoric Cauchy 
stress tensor as 
and pressure 
∇𝑛+1
2⁄
𝑠𝑖𝑗
= 2𝐺𝜀̇𝑖𝑗
′ 𝑛+1
2⁄ ,
𝑝𝑛+1 = −𝐾ln𝑉𝑛+1,
(22.1.1)
(22.1.2)
where 𝐺 and 𝐾 are the elastic shear and bulk moduli, respectively, and 𝑉 is the relative 
volume, i.e., the ratio of the current volume to the initial volume.
LS-DYNA Theory Manual 
Material Models 
22.2  Material Model 2:  Orthotropic Elastic 
The  material  law  that  relates  second  Piola-Kirchhoff  stress  𝐒  to  the  Green-St.  
Venant strain 𝐄 is 
𝐒 = 𝐂 ⋅ 𝐄 = 𝐓T𝐂l𝐓 ⋅ 𝐄,
where 𝐓 is the transformation matrix [Cook 1974]. 
𝐓 =
𝑙1
⎡
⎢
𝑙2
⎢
⎢
𝑙3
⎢
⎢
2𝑙1𝑙2
⎢
2𝑙2𝑙3
⎢
2𝑙3𝑙1
⎣
𝑚1
𝑚2
𝑚3
2𝑚1𝑚2
2𝑚2𝑚3
2𝑚3𝑚1
𝑛1
𝑛2
𝑛3
2𝑛1𝑛2
2𝑛2𝑛3
2𝑛3𝑛1
𝑙1𝑚1
𝑙2𝑚2
𝑙3𝑚3
(𝑙1𝑚2 + 𝑙1𝑚1)
(𝑙2𝑚3 + 𝑙3𝑚2)
(𝑙3𝑚1 + 𝑙1𝑚3)
𝑚1𝑛1
𝑚2𝑛2
𝑚3𝑛3
(𝑚1𝑛2 + 𝑚2𝑛1)
(𝑚2𝑛3 + 𝑚3𝑛2)
(𝑚3𝑛1 + 𝑚1𝑛3)
𝑛1𝑙1
⎤
⎥
𝑛2𝑙2
⎥
⎥
𝑛3𝑙3
⎥
⎥
(𝑛1𝑙2 + 𝑛2𝑙1)
⎥
(𝑛2𝑙3 + 𝑛3𝑙2)
⎥
(𝑛3𝑙1 + 𝑛1𝑙3)⎦
, 
𝑙𝑖, 𝑚𝑖, 𝑛𝑖 are the direction cosines 
(22.2.1)
(22.2.2)
(22.2.3)
′ denotes the material axes.  The constitutive matrix 𝐂l is defined in terms of the 
′ = 𝑙𝑖𝑥1 + 𝑚𝑖𝑥2 + 𝑛𝑖𝑥3,
𝑥𝑖
𝑖 = 1, 2, 3,
and 𝑥𝑖
material axes as 
−1 =
𝐂l
𝐸11
𝜐12
𝐸11
𝜐13
𝐸11
−
−
𝜐21
𝐸22
𝐸22
𝜐23
𝐸22
−
−
𝜐31
𝐸33
𝜐32
𝐸33
𝐸33
𝐺12
𝐺23
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
, 
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
𝐺31⎦
−
−
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
where the subscripts denote the material axes, i.e., 
𝜐𝑖𝑗 = 𝜐𝑥𝑖
′
′𝑥𝑗
and
′.
𝐸𝑖𝑖 = 𝐸𝑥𝑖
Since 𝐂l is symmetric 
𝜐12
𝐸11
=
𝜐21
𝐸22
, etc.
The vector of Green-St.  Venant strain components is 
𝐄T = [𝐸11 𝐸22 𝐸33 𝐸12 𝐸23 𝐸31].
(22.2.4)
(22.2.5)
(22.2.6)
(22.2.7)
Material Models 
LS-DYNA Theory Manual 
After  computing  𝑆𝑖𝑗,  we  use  Equation  (21.32)  to  obtain  the  Cauchy  stress.    This 
model will predict realistic behavior for finite displacement and rotations as long as the 
strains are small.
LS-DYNA Theory Manual 
Material Models 
22.3  Material Model 3:  Elastic Plastic with Kinematic 
Hardening 
Isotropic, kinematic, or a combination of isotropic and kinematic hardening may 
be obtained by varying a parameter, called 𝛽 between 0 and 1.  For 𝛽 equal to 0 and 1, 
respectively, kinematic and isotropic hardening are obtained as shown in Figure 22.3.1.  
Krieg and Key [1976] formulated this model and the implementation is based on their 
paper. 
In isotropic hardening, the center of the yield surface is fixed but the radius is a 
function of the plastic strain.  In kinematic hardening, the radius of the yield surface is 
fixed  but  the  center  translates  in  the  direction  of  the  plastic  strain.    Thus  the  yield 
condition is 
where 
𝜙 =
𝜉𝑖𝑗𝜉𝑖𝑗 −
𝜎𝑦
= 0,
𝜉𝑖𝑗 = 𝑠𝑖𝑗 − 𝛼𝑖𝑗
p .
𝜎𝑦 = 𝜎0 + 𝛽𝐸p𝜀eff
The co-rotational rate of 𝛼𝑖𝑗 is 
∇ = (1 − 𝛽)
𝛼𝑖𝑗
p.
𝐸p𝜀̇𝑖𝑗
Hence, 
𝑛+1 = 𝛼𝑖𝑗
𝛼𝑖𝑗
𝑛 + (𝛼𝑖𝑗
∇𝑛+1
2⁄
𝑛+1
2⁄
+ 𝛼𝑖𝑘
𝑛 𝛺𝑘𝑗
𝑛+1
2⁄
+ 𝛼𝑗𝑘
𝑛 𝛺𝑘𝑖
(22.3.1)
(22.3.2)
(22.3.3)
(22.3.4)
(22.3.5)
) Δ𝑡𝑛+1
2⁄ .
Strain  rate  is  accounted  for  using  the  Cowper-Symonds  [Jones  1983]  model 
which scales the yield stress by a strain rate dependent factor  
⎤
⎥
⎦
where 𝑝 and 𝐶 are user defined input constants and 𝜀̇ is the strain rate defined as: 
(𝜎0 + 𝛽𝐸p𝜀eff
𝜎𝑦 =
1 + (
p ),
⎡
⎢
⎣
)
𝜀̇
𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗.
(22.3.6)
(22.3.7)
Material Models 
LS-DYNA Theory Manual 
δx
Yield
Stress
⎛
⎜
⎝
⎛
⎜
⎝
l0
ln
β=0, kinematic hardening
β=1, isotropic hardening
Figure 22.3.1.  Elastic-plastic behavior with isotropic and kinematic hardening 
where  l0  and  l  are  the  undeformed  and  deformed  length  of  uniaxial  tension
specimen, respectively. 
The current radius of the yield surface, 𝜎𝑦, is the sum of the initial yield strength, 
p , where 𝐸p is the plastic hardening modulus 
𝜎0, plus the growth 𝛽𝐸p𝜀eff
and  𝜀eff
p  is the effective plastic strain 
𝐸p =
𝐸t𝐸
𝐸 − 𝐸t
,
p = ∫ (
𝜀eff
2⁄
p)
p𝜀̇𝑖𝑗
𝜀̇𝑖𝑗
𝑑𝑡
.
(22.3.8)
(22.3.9)
The  plastic  strain  rate  is  the  difference  between  the  total  and  elastic  (right 
superscript e) strain rates: 
p = 𝜀̇𝑖𝑗 − 𝜀̇𝑖𝑗
e .
𝜀̇𝑖𝑗
(22.3.10)
In the implementation of this material model, the deviatoric stresses are updated 
elastically, as described for model 1, but repeated here for the sake of clarity: 
∗ = 𝜎𝑖𝑗
𝜎𝑖𝑗
𝑛 + 𝐶𝑖𝑗𝑘𝑙Δ𝜀𝑘𝑙,
(22.3.11)
where 
∗ 
𝜎𝑖𝑗
𝑛 
𝜎𝑖𝑗
C𝑖𝑗𝑘𝑙 
is the trial stress tensor, 
is the stress tensor from the previous time step, 
is the elastic tangent modulus matrix,
LS-DYNA Theory Manual 
Material Models 
Δ𝜀𝑘𝑙 
is the incremental strain tensor. 
and,  if  the  yield  function  is  satisfied,  nothing  else  is  done.    If,  however,  the  yield 
function  is  violated,  an  increment  in  plastic  strain  is  computed,  the  stresses  are  scaled 
back to the yield surface, and the yield surface center is updated.   
Let s𝑖𝑗
∗  represent the trial elastic deviatoric stress state at 𝑛 + 1  
and 
∗ = σ𝑖𝑗
s𝑖𝑗
∗ −
∗ ,
σ𝑘𝑘
∗ = s𝑖𝑗
ξ𝑖𝑗
∗ − α𝑖𝑗.
Define the yield function,  
(22.3.12)
(22.3.13)
𝜙 =
∗𝜉𝑖𝑗
𝜉𝑖𝑗
∗ − 𝜎𝑦
2 = 𝛬2 − 𝜎𝑦
2 {
≤ 0
> 0
for elastic or neutral loading
for plastic harding
, 
(22.3.14)
For plastic hardening then 
p𝑛+1
𝜀eff
p𝑛
= 𝜀eff
+
𝛬 − 𝜎𝑦
3𝐺 + 𝐸p
p𝑛
= 𝜀eff
p ,
+ Δ𝜀eff
scale back the stress deviators  
and update the center: 
𝑛+1 = 𝜎𝑖𝑗
𝜎𝑖𝑗
∗ −
3𝐺Δ𝜀eff
∗,
𝜉𝑖𝑗
𝑛 + 1 = 𝛼𝑖𝑗
𝛼𝑖𝑗
𝑛 +
(1 − 𝛽)𝐸pΔ𝜀eff
∗.
𝜉𝑖𝑗
(22.3.15)
(22.3.16)
(22.3.17)
Plane Stress Plasticity 
The plane stress plasticity options apply to beams, shells, and thick shells.  Since 
the stresses and strain increments are transformed to the lamina coordinate system for 
the  constitutive  evaluation,  the  stress  and  strain  tensors  are  in  the  local  coordinate 
system.  
The  application  of  the  Jaumann  rate  to  update  the  stress  tensor  allows  for  the 
possibility  that  the  normal  stress,  𝜎33,  will  not  be  zero.    The  first  step  in  updating  the 
stress  tensor  is  to  compute  a  trial  plane  stress  update  assuming  that  the  incremental 
strains  are  elastic.    In  the  above,  the  normal  strain  increment  Δ𝜀33  is  replaced  by  the 
elastic strain increment 
Δ𝜀33 = −
𝜎33 + 𝜆(Δ𝜀11 + Δ𝜀22)
𝜆 + 2𝜇
,
(22.3.18)
where 𝜆 and 𝜇 are Lamé’s constants.
Material Models 
LS-DYNA Theory Manual 
When the trial stress is within the yield surface, the strain increment is elastic and 
the  stress  update  is  completed.    Otherwise,  for  the  plastic  plane  stress  case,  secant 
iteration  is  used  to  solve  Equation  (22.3.16) for  the  normal  strain  increment  (Δ𝜀33) 
required to produce a zero normal stress: 
𝑖 = 𝜎33
𝜎33
∗ −
p𝑖
3𝐺Δ𝜀eff
𝜉33
,
(22.3.19)
Here, the superscript 𝑖 indicates the iteration number. 
The secant iteration formula for Δε33 (the superscript p is dropped for clarity) is 
𝑖−1
𝑖 − Δ𝜀33
Δ𝜀33
𝑖−1 𝜎33
𝑖 − 𝜎33
𝜎33
where  the  two  starting  values  are  obtained  from  the  initial  elastic  estimate  and  by 
assuming a purely plastic increment, i.e., 
𝑖+1 = Δ𝜀33
𝑖−1 −
(22.3.20)
Δ𝜀33
𝑖−1,
1 = −(Δ𝜀11 − Δ𝜀22).
These starting values should bound the actual values of the normal strain increment. 
Δ𝜀33
(22.3.21)
The iteration procedure uses the updated normal stain increment to update first 
the deviatoric stress and then the other quantities needed to compute the next estimate 
of the normal stress in Equation (22.3.19).  The iterations proceed until the normal stress 
 is sufficiently small.  The convergence criterion requires convergence of the normal 
𝜎33
strains: 
∣Δ𝜀33
𝑖 − Δ𝜀33
𝑖−1∣
𝑖+1∣
∣Δ𝜀33
< 10−4.
(22.3.22)
After  convergence,  the  stress  update  is  completed  using  the  relationships  given  in 
Equations (22.3.16) and (22.3.17)
LS-DYNA Theory Manual 
Material Models 
22.4  Material Model 4:  Thermo-Elastic-Plastic 
This  model  was  adapted  from  the  NIKE2D  [Hallquist  1979]  code.    A  more 
complete description of its formulation is given in the NIKE2D user’s manual. 
Letting 𝑇  represent  the temperature,  we  compute  the  elastic  co-rotational  stress 
rate as 
where 
∇ = 𝐶𝑖𝑗𝑘𝑙(𝜀̇𝑘𝑙 − ε̇𝑘𝑙
𝜎𝑖𝑗
T ) + 𝜃̇
𝑖𝑗𝑑𝑇,
𝜃̇
𝑖𝑗 =
𝑑𝐶𝑖𝑗𝑘𝑙
𝑑𝑇
−1 𝜎̇𝑚𝑛,
𝐶𝑘𝑙𝑚𝑛
and 𝐶𝑖𝑗𝑘𝑙 is the temperature dependent elastic constitutive matrix: 
𝐶𝑖𝑗𝑘𝑙 =
(1 + 𝜐)(1 − 2𝜐)
⎡1 − 𝜐
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
1 − 𝜐
1 − 𝜐
1 − 2𝜐
1 − 2𝜐
1 − 2𝜐
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
, 
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎦
(22.4.1)
(22.4.2)
(22.4.3)
where  𝜐  is  Poisson’s  ratio.    The  thermal  strain  rate  can  be  written  in  terms  of  the 
coefficient of thermal expansion 𝛼 as: 
T = 𝛼𝑇̇𝛿𝑖𝑗,
𝜀̇𝑖𝑗
(22.4.4)
When  treating  plasticity,  we  use  a  procedure  analogous  to  that  for  material  3.  
We  update  the  stresses  elastically  and  check  to  see  if  we  violate  the  isotropic  yield 
function 
where 
𝜙 =
𝑠𝑖𝑗𝑠𝑖𝑗 −
𝜎𝑦(𝑇)2
,
p .
𝜎𝑦(𝑇) = 𝜎𝑜(𝑇) + 𝐸p(𝑇)𝜀eff
(22.4.5)
(22.4.6)
Material Models 
LS-DYNA Theory Manual 
The  initial  yield,  𝜎o,  and  plastic  hardening  modulus,  𝐸p,  are  temperature 
dependent.  If the behavior is elastic we do nothing; otherwise, we scale back the stress 
deviators by the factor 𝑓s: 
where 
𝑛+1 = 𝑓s𝑠𝑖𝑗
∗ ,
𝑠𝑖𝑗
𝑓s =
𝜎𝑦
2⁄
∗ )
∗ 𝑠𝑖𝑗
𝑠𝑖𝑗
(3
,
and update the plastic strain by the increment 
p =
Δ𝜀eff
2⁄
(1 − 𝑓s)(3
∗ )
∗ 𝑠𝑖𝑗
𝑠𝑖𝑗
𝐺 + 3𝐸p
.
(22.4.7)
(22.4.8)
(22.4.9)
LS-DYNA Theory Manual 
Material Models 
22.5  Material Model 5:  Soil and Crushable Foam 
This  model,  due  to  Krieg  [1972],  provides  a  simple  model  for  foam  and  soils 
whose  material  properties  are  not  well  characterized.    We  believe  the  other  foam 
models in LS-DYNA are superior in their performance and are recommended over this 
model which simulates the crushing through the volumetric deformations.  If the yield 
stress is too low, this foam model gives nearly fluid like behavior. 
A pressure-dependent flow rule governs the deviatoric behavior: 
𝜙s =
s𝑖𝑗s𝑖𝑗 − (𝑎0 + 𝑎1𝑝 + 𝑎2𝑝2),
(22.5.1)
where 𝑎0, 𝑎1, and 𝑎2 are user-defined constants.  Volumetric yielding is determined by a 
tabulated curve of pressure versus volumetric strain.  Elastic unloading from this curve 
is assumed to a tensile cutoff as illustrated in Figure 22.5.1. 
Implementation  of  this  model  is  straightforward.    One  history  variable,  the 
maximum  volumetric  strain  in  compression,  is  stored.    If  the  new  compressive 
volumetric  strain  exceeds  the  stored  value,  loading  is  indicated.    When  the  yield 
∗ , are scaled back using a simple radial 
condition is violated, the updated trial stresses, 𝑠𝑖𝑗
Loading and unloading (along the 
grey arows) follows the input curve 
when the volumetric crushing option 
is off (VCR = 1.0)
tension
compression
Volumetric Strain,
ln
⎛
⎜
⎝
⎛
⎜
V0
⎝
Pressure Cutoff Value
The bulk unloading modulus is used
if the volumetric crushing option is on 
(VCR = 0).  In thiscase the aterial's response
follows the black arrows.
Figure 22.5.1.  Volumetric strain versus pressure curve for soil and crushable 
foam model. 
return algorithm:
Material Models 
LS-DYNA Theory Manual 
𝑛+1 =
s𝑖𝑗
⎜⎜⎜⎛𝑎0 + 𝑎1𝑝 + a2𝑝2
s𝑖𝑗s𝑖𝑗
⎝
2⁄
⎟⎟⎟⎞
⎠
∗ . 
s𝑖𝑗
(22.5.2)
If the hydrostatic tension exceeds the cutoff value, the pressure is set to the cutoff 
value and the deviatoric stress tensor is zeroed.
LS-DYNA Theory Manual 
Material Models 
22.6  Material Model 6:  Viscoelastic 
In  this  model,  linear  viscoelasticity  is  assumed  for  the  deviatoric  stress  tensor 
[Herrmann and Peterson 1968]: 
where 
𝑠𝑖𝑗 = 2 ∫ 𝜙(𝑡 − 𝜏)
′ (𝜏)
∂𝜀𝑖𝑗
∂𝜏
𝑑𝜏
,
𝜙(𝑡) = G∞ + (G0 − G∞)𝑒−𝛽𝑡,
(22.6.1)
(22.6.2)
is the shear relaxation modulus.  A recursion formula is used to compute the new value 
of the hereditary integral at time 𝑡𝑛+1 from its value at time 𝑡𝑛.  Elastic bulk behavior is 
assumed: 
𝑝 = 𝐾ln𝑉,
(22.6.3)
where pressure is integrated incrementally.
Material Models 
LS-DYNA Theory Manual 
22.7  Material Model 7:  Continuum Rubber 
The  hyperelastic  continuum  rubber  model  was  studied  by  Blatz  and  Ko  [1962].  
In this model, the second Piola-Kirchhoff stress is given by 
𝑆𝑖𝑗 = 𝐺 (𝑉 −1𝐶𝑖𝑗 − 𝑉
− 1
1−2𝜐𝛿𝑖𝑗),
(22.7.1)
where 𝐺 is the shear modulus, 𝑉 is the relative volume, 𝜐 is Poisson’s  ratio, and 𝐶𝑖𝑗 is 
the right Cauchy-Green strain: 
C𝑖𝑗 =
𝜕𝑥𝑘
𝜕𝑋𝑖
𝜕𝑥𝑘
𝜕𝑋𝑗
,
(22.7.2)
after determining 𝑆𝑖𝑗, it is transformed into the Cauchy stress tensor, 𝜎𝑖𝑗: 
𝜕𝑥𝑗
𝜕𝑋𝑙
where 𝜌0 and 𝜌 are the initial and current density, respectively.  The default value of υ is 
0.463.
𝜕𝑥𝑖
𝜕𝑋𝑘
𝜎𝑖𝑗 =
𝜌0
(22.7.3)
𝑆𝑘𝑙,
LS-DYNA Theory Manual 
Material Models 
22.8  Material Model 8:  Explosive Burn 
Burn fractions, which multiply the equations of states for high explosives, control 
the release of chemical energy for simulating detonations.  In the initialization phase, a 
lighting  time  𝑡1    is  computed  for  each  element  by  dividing  the  distance  from  the 
detonation point to the center of the element by the detonation velocity 𝐷.  If multiple 
detonation  points  are  defined,  the  closest  point  determines  𝑡1.  The  burn  fraction  𝐹  is 
taken as the maximum 
𝐹 = max(𝐹1, 𝐹2),
(22.8.1)
where 
𝐹1 =
)
3   (
𝑣e
𝐴emax
⎧ 2 (𝑡 − 𝑡𝑙)𝐷
{
{
{{
{
⎨
{{
{
{{
⎩
 0
𝐹2 =
1 − 𝑉
1 − 𝑉CJ
,
𝑡 > 𝑡l
 𝑡  ≤ 𝑡l
(22.8.2)
(22.8.3)
where 𝑉CJ is the Chapman-Jouguet relative volume and 𝑡 is current time.  If 𝐹 exceeds 1, 
it is reset to 1.  This calculation of the burn fraction usually requires several time steps 
for  𝐹  to  reach  unity,  thereby  spreading  the  burn  front  over  several  elements.    After 
reaching  unity, 𝐹  is  held  constant.    This  burn  fraction  calculation  is  based  on  work  by 
Wilkins [1964] and is also discussed by Giroux [1973]. 
As  an  option,  the  high  explosive  material  can  behave  as  an  elastic  perfectly-
plastic solid prior to detonation.  In this case we update the stress tensor, to an elastic 
trial stress, 𝑠𝑖𝑗
∗𝑛+1,  
∗𝑛+1 = 𝑠𝑖𝑗
𝑠𝑖𝑗
𝑛 + 𝑠𝑖𝑝𝛺𝑝𝑗 + 𝑠𝑗𝑝𝛺𝑝𝑖 + 2𝐺𝜀̇𝑖𝑗
′ 𝑑𝑡,
(22.8.4)
where 𝐺 is the shear modulus, and 𝜀̇𝑖𝑗
condition is given by: 
′  is the deviatoric strain rate.  The von Mises yield 
𝜎𝑦
where  the  second  stress  invariant,  𝐽2,  is  defined  in  terms  of  the  deviatoric  stress 
components as 
𝜙 = 𝐽2 −
(22.8.5)
,
𝐽2 =
𝑠𝑖𝑗𝑠𝑖𝑗,
(22.8.6)
Material Models 
LS-DYNA Theory Manual 
and the yield stress is 𝜎𝑦.  If yielding has occurred, i.e., 𝜙 > 0, the deviatoric trial stress 
is scaled to obtain the final deviatoric stress at time 𝑛 + 1: 
If 𝜙 ≤ 0, then 
𝑛+1 =
𝑠𝑖𝑗
𝜎𝑦
√3𝐽2
∗𝑛+1,
𝑠𝑖𝑗
𝑛+1 = 𝑠𝑖𝑗
𝑠𝑖𝑗
∗𝑛+1.
Before detonation pressure is given by the expression 
𝑝𝑛+1 = 𝐾 (
𝑉𝑛+1 − 1).
where K is the bulk modulus.  Once the explosive material detonates: 
and the material behaves like a gas. 
𝑛+1 = 0.
𝑠𝑖𝑗
(22.8.7)
(22.8.8)
(22.8.9)
(22.8.10)
The  shadow  burn  option  should  be  active  when  computing  the  lighting  time  if 
there exist elements within the mesh for which there is no direct line of sight from the 
detonation  points.    The  shadow  burn  option  is  activated  in  the  control  section.    The 
lighting time is based  on the shortest distance through the explosive material.  If inert 
obstacles exist within the explosive material, the lighting time will account for the extra 
time required for the detonation wave to travel around the obstacles.  The lighting times 
also  automatically  accounts  for  variations  in  the  detonation  velocity  if  different 
explosives  are  used.    No  additional  input  is  required  for  the  shadow  option  but  care 
must  be  taken  when  setting  up  the  input.    This  option  works  for  two  and  three-
dimensional solid elements.  It is recommended that for best results: 
1.  Keep the explosive mesh as uniform as possible with elements of roughly the 
same dimensions.   
2. 
3. 
Inert  obstacle  such  as  wave  shapers  within  the  explosive  must  be  somewhat 
larger  than the  characteristic  element  dimension  for  the  automatic  tracking  to 
function properly.  Generally, a factor of two should suffice.  The characteristic 
element dimension is found by checking all explosive elements for the largest 
diagonal  
The  detonation  points  should  be  either  within  or  on  the  boundary  of  the 
explosive.  Offset points may fail to initiate the explosive. 
4.  Check  the  computed  lighting  times  in  the  post  processor  LS-PrePost.    The 
lighting times may be displayed at time = 0, state 1, by plotting component 7 (a 
component normally reserved for plastic strain) for the explosive material.  The 
lighting  times  are  stored  as  negative  numbers.    The  negative  lighting  time  is 
replaced by the burn fraction when the element ignites.
LS-DYNA Theory Manual 
Material Models 
5. 
Line  detonations  may  be  approximated  by  using  a  sufficient  number  of 
detonation points to define the line.  Too many detonation points may result in 
significant initialization cost.
Material Models 
LS-DYNA Theory Manual 
22.9  Material Model 9:  Null Material 
For  solid  elements  equations  of  state  can  be  called  through  this  model  to  avoid 
deviatoric stress calculations.  A pressure cutoff may be specified to set a lower bound 
on  the  pressure.    This  model  has  been  very  useful  when  combined  with  the  reactive 
high  explosive  model  where  material  strength  is  often  neglected.    The  null  material 
should not be used to delete solid elements.   
An optional viscous stress of the form 
′ ,
𝜎𝑖𝑗 = 𝜇𝜀̇𝑖𝑗
′  is the deviatoric strain rate.   
is computed for nonzero 𝜇 where 𝜀̇𝑖𝑗
(22.9.1)
Sometimes it is advantageous to model contact surfaces via shell elements which 
are  not  part of  the  structure,  but  are  necessary  to  define  areas  of  contact  within  nodal 
rigid bodies or between nodal rigid bodies.  Beams and shells that use this material type 
are  completely  bypassed  in  the  element  processing.    The  Young’s  modulus  and 
Poisson’s  ratio  are  used  only  for  setting  the  contact  interface  stiffnesses,  and  it  is 
recommended that reasonable values be input.
LS-DYNA Theory Manual 
Material Models 
22.10  Material Model 10:  Elastic-Plastic-Hydrodynamic 
For completeness we give the entire derivation of this constitutive model based 
on radial return plasticity.   
The  pressure,  𝑝,  deviatoric  strain  rate,  𝜀̇𝑖𝑗
strain rate, and 𝜀̇v, are defined in Equation (1.1.1): 
′ ,  deviatoric  stress  rate,  𝑠 ̇𝑖𝑗,  volumetric 
𝜎𝑖𝑗𝛿𝑖𝑗
𝑝 = −
𝑠𝑖𝑗 = 𝜎𝑖𝑗 + 𝑝𝛿𝑖𝑗
∇ = 2𝜇𝜀̇𝑖𝑗
𝑠𝑖𝑗
′ = 𝜀̇𝑖𝑗 −
𝜀̇𝑖𝑗
𝜀̇v = 𝜀̇𝑖𝑗𝛿𝑖𝑗 
′ .
′ = 2𝐺𝜀̇𝑖𝑗
𝜀̇v
The Jaumann rate of the deviatoric stress, 𝑠𝑖𝑗
∇, is given by: 
∇ = 𝑠 ̇𝑖𝑗 − 𝑠𝑖𝑝𝛺𝑝𝑗 − 𝑠𝑗𝑝𝛺𝑝𝑖.
𝑠𝑖𝑗
First we update s𝑖𝑗
𝑛+1 = 𝑠𝑖𝑗
𝑖𝑗
∗
𝑠 
𝑛 to s𝑖𝑗
𝑛+1 elastically 
𝑛 + 𝑠𝑖𝑝𝛺𝑝𝑗 + 𝑠𝑗𝑝𝛺𝑝𝑖 + 2𝐺𝜀̇𝑖𝑗
′ 𝑑𝑡 = 𝑠𝑖𝑗
𝑛 + 𝑅𝑖𝑗⏟
𝑅𝑛
𝑠𝑖𝑗
(22.10.1)
(22.10.2)
(22.10.3)
′ 𝑑𝑡⏟
+ 2𝐺𝜀̇𝑖𝑗
′
2𝐺Δ𝜀𝑖𝑗
, 
where  the  left  superscript,  *,  denotes  a  trial  stress  value.    The  effective  trial  stress  is 
defined by 
𝑠∗ = (
𝑠∗
𝑛+1 𝑠∗
𝑖𝑗
𝑛+1)
𝑖𝑗
2⁄
,
and if 𝑠∗ exceeds yield stress 𝜎y, the Von Mises flow rule: 
𝜙 =
𝑠𝑖𝑗𝑠𝑖𝑗 −
𝜎y
≤ 0,
(22.10.4)
(22.10.5)
is violated and we scale the trial stresses back to the yield surface, i.e., a radial return 
𝑛+1 =
𝑠𝑖𝑗
𝜎𝑦
𝑠∗ 𝑠∗
𝑛+1 = 𝑚 𝑠∗
𝑖𝑗
𝑛+1.
𝑖𝑗
(22.10.6)
The  plastic  strain  increment  can  be  found  by  subtracting  the  deviatoric  part  of 
R𝑛
𝑛+1 − 𝑠𝑖𝑗
), from the total deviatoric increment, 
the strain increment that is elastic,  1
Δε𝑖𝑗
′ , i.e., 
2𝐺 (𝑠𝑖𝑗
p = Δ𝜀𝑖𝑗
′ −
Δ𝜀𝑖𝑗
2𝐺
 R𝑛
𝑛+1 − 𝑠𝑖𝑗
(𝑠𝑖𝑗
).
(22.10.7)
Material Models 
LS-DYNA Theory Manual 
Recalling that,  
′ =
Δ𝜀𝑖𝑗
∗
( 𝑠 
R𝑛
𝑛+1 − 𝑠𝑖𝑗
𝑖𝑗
2𝐺
)
,
and substituting Equation (22.10.8) into (22.10.7) we obtain, 
p =
Δ𝜀𝑖𝑗
∗
( 𝑠 
𝑛+1 − 𝑠𝑖𝑗
𝑖𝑗
2𝐺
𝑛+1)
.
Substituting Equation (22.10.6)  
𝑛+1 = 𝑚 𝑠∗
𝑠𝑖𝑗
𝑛+1,
𝑖𝑗
into Equation (22.10.9) gives, 
p = (
Δ𝜀𝑖𝑗
1 − 𝑚
2𝐺
) 𝑠∗
𝑛+1 =
𝑖𝑗
1 − 𝑚
2𝐺𝑚
𝑛+1 = 𝑑λ𝑠𝑖𝑗
𝑠𝑖𝑗
𝑛+1.
By definition an increment in effective plastic strain is 
Δ𝜀p = (
2⁄
p)
pΔ𝜀𝑖𝑗
Δ𝜀𝑖𝑗
.
Squaring both sides of Equation (22.10.11) leads to: 
Δ𝜀𝑖𝑗
pΔ𝜀𝑖𝑗
p   = (
1 − 𝑚
2𝐺
)
𝑠∗
𝑛+1 𝑠∗
𝑖𝑗
𝑛+1
𝑖𝑗
or from Equations (22.10.4) and (22.10.12): 
Hence, 
Δ𝜀p2
= (
1 − 𝑚
2𝐺
2 2
)
𝑠∗2
Δ𝜀p =
1 − 𝑚
3𝐺
𝑠∗ =
𝑠∗ − 𝜎y
3𝐺
where we have substituted for m from Equation (22.10.6) 
𝑚 =
𝜎y
𝑠∗
If isotropic hardening is assumed then: 
𝑛+1 = 𝜎y
𝜎y
𝑛 + 𝐸pΔ𝜀p
and from Equation (22.10.15) 
Δ𝜀p =
𝑛+1)
(𝑠∗ − 𝜎y
3𝐺
=
(𝑠∗ − 𝜎y
𝑛 − 𝐸pΔ𝜀p)
.
3𝐺
Thus, 
(22.10.8)
(22.10.9)
(22.10.10)
(22.10.11)
(22.10.12)
(22.10.13)
(22.10.14)
(22.10.15)
(22.10.16)
(22.10.17)
(22.10.18)
LS-DYNA Theory Manual 
Material Models 
and solving for the incremental plastic strain gives 
(3𝐺 + 𝐸p)Δ𝜀p = (𝑠∗ − 𝜎y
𝑛),
Δ𝜀p =
𝑛)
(𝑠∗ − 𝜎y
.
(3𝐺 + 𝐸p)
(22.10.19)
(22.10.20)
The algorithm for plastic loading can now be outlined in five simple stress.  If the 
effective trial stress exceeds the yield stress then 
1. 
Solve for the plastic strain increment: 
𝑛)
(𝑠∗ − σy
.
(3𝐺 + 𝐸p)
Δ𝜀p =
2.  Update the plastic strain: 
𝜀p𝑛+1
= 𝜀p𝑛
+ Δ𝜀p.
3.  Update the yield stress: 
𝑛+1 = 𝜎y
𝜎y
𝑛 + 𝐸pΔ𝜀p.
4.  Compute the scale factor using the yield strength at time 𝑛 + 1: 
𝑚 =
𝑛+1
𝜎y
𝑠∗ .
5.  Radial return the deviatoric stresses to the yield surface: 
𝑛+1 = 𝑚 𝑠∗
𝑠𝑖𝑗
𝑛+1.
𝑖𝑗
(22.10.21)
(22.10.22)
(22.10.23)
(22.10.24)
(22.10.25)
Material Models 
LS-DYNA Theory Manual 
22.11  Material Model 11:  Elastic-Plastic With Thermal 
Softening 
Steinberg and Guinan [1978] developed this model for treating plasticity at high 
strain rates (105 s-1) where enhancement of the yield strength due to strain rate effects is 
saturated out. 
Both  the  shear  modulus  𝐺  and  yield  strength  𝜎y  increase  with  pressure  but 
decrease  with  temperature.    As  a  melt  temperature  is  reached,  these  quantities 
approach zero.  We define the shear modulus before the material melts as 
𝐺 = 𝐺0 [1 + 𝑏𝑝𝑉
3⁄ − ℎ (
𝐸 − 𝐸c
3𝑅′
− 300)] 𝑒
−
𝑓𝐸
𝐸m−𝐸,
where 𝐺0, 𝑏, ℎ, and 𝑓  are input parameters, 𝐸c is the cold compression energy: 
𝐸c(𝑋) = ∫ 𝑝𝑑𝑥
−
900𝑅′exp(𝑎𝑥)
2(𝛾𝑜−𝑎−1
)
(1 − 𝑋)
,
where, 
𝑋 = 1 − 𝑉,
and 𝐸m is the melting energy: 
𝐸m(𝑋) = 𝐸c(𝑋) + 3𝑅′𝑇m(𝑋),
which is a function of the melting temperature 𝑇m(𝑋): 
𝑇m(𝑋) =
𝑇moexp(2𝑎𝑋)
2(𝛾𝑜−𝑎−1
)
(1 − 𝑋)
,
(22.11.1)
(22.11.2)
(22.11.3)
(22.11.4)
(22.11.5)
and  the  melting  temperature  𝑇mo  at  𝜌 = 𝜌0.    The  constants  𝛾0  and  a  are  input 
parameters.  In the above equation, 𝑅′ is defined by 
𝑅′ =
𝑅𝜌0
,
(22.11.6)
where 𝑅 is the gas constant and A is the atomic weight.  The yield strength 𝜎y is given 
by: 
𝜎y = 𝜎0
′ [1 + 𝑏′𝑝𝑉
3 − ℎ (
𝐸 − 𝐸c
3𝑅′
− 300)] 𝑒
−
𝑓𝐸
𝐸m−𝐸.
If 𝐸m exceeds 𝐸𝑖.  Here, 𝜎0
′   is given by: 
′ = 𝜎0[1 + 𝛽(𝛾𝑖 + 𝜀̅𝑝)]𝑛.
𝜎0
(22.11.7)
(22.11.8)
LS-DYNA Theory Manual 
Material Models 
where  𝛾1  is  the  initial  plastic  strain,  and  𝑏′  and  𝜎0
exceeds 𝜎max, the maximum permitted yield strength, 𝜎0
the material melts, 𝜎y and 𝐺 are set to zero. 
′  
′   are  input  parameters.    Where  𝜎0
′  is set to equal to 𝜎max.  After 
LS-DYNA fits the cold compression energy to a ten-term polynomial expansion: 
𝜂𝑖,
(22.11.9)
𝐸c = ∑ 𝐸𝐶𝑖
𝑖=0
𝜌0
where 𝐸𝐶𝑖 is the ith coefficient and 𝜂 =
the fit [Kreyszig 1972].  The ten coefficients may also be specified in the input. 
.  The least squares method is used to perform 
Once the yield strength and shear modulus are known, the numerical treatment 
is similar to that for material model 10.
Material Models 
LS-DYNA Theory Manual 
22.12  Material Model 12:  Isotropic Elastic-Plastic 
The von Mises yield condition is given by: 
𝜎y
where  the  second  stress  invariant,  𝐽2,  is  defined  in  terms  of  the  deviatoric  stress 
components as 
𝜙 = 𝐽2 −
(22.12.1)
,
𝐽2 =
𝑠𝑖𝑗𝑠𝑖𝑗,
(22.12.2)
and  the  yield  stress, 𝜎y,  is  a  function  of  the  effective  plastic  strain, 𝜀eff
hardening modulus, 𝐸p: 
p ,  and  the  plastic 
p .
𝜎y = 𝜎0 + 𝐸p𝜀eff
(22.12.3)
The effective plastic strain is defined as 
p = ∫ 𝑑𝜀eff
𝜀eff
,
(22.12.4)
p = √2
where  𝑑𝜀eff
input tangent modulus, 𝐸t, as 
3 𝑑𝜀𝑖𝑗
p𝑑𝜀𝑖𝑗
p,  and  the  plastic  tangent  modulus  is  defined  in  terms  of  the 
𝐸p =
𝐸𝐸t
𝐸 − 𝐸t
.
(22.12.5)
Pressure is given by the expression 
𝑉𝑛+1 − 1),
where 𝐾 is the bulk modulus.  This is perhaps the most cost effective plasticity model.  
Only one history variable, 𝜀eff
p , is stored with this model. 
𝑝𝑛+1 = 𝐾 (
(22.12.6)
This  model  is  not  recommended  for  shell  elements.    In  the  plane  stress 
implementation,  a  one-step  radial  return  approach  is  used  to  scale  the  Cauchy  stress 
tensor to if the state of stress exceeds the yield surface.  This approach to plasticity leads 
to inaccurate shell thickness updates and stresses after yielding.  This is the only model 
in LS-DYNA for plane stress that does not default to an iterative approach.
LS-DYNA Theory Manual 
Material Models 
22.13  Material Model 13:  Isotropic Elastic-Plastic with 
Failure 
This highly simplistic failure model is occasionally useful.  Material model 12 is 
called to update the stress tensor.  Failure is initially assumed to occur if either  
𝑝𝑛+1 < 𝑝min,
(22.13.1)
or 
p > 𝜀max
𝜀eff
,
(22.13.2)
where 𝑝min and 𝜀max
may never be negative and the deviatoric components are set to zero: 
 are user-defined parameters.  Once failure has occurred, pressure 
for all time.  The failed element can only carry loads in compression.
𝑠𝑖𝑗 = 0
(22.13.3)
Material Models 
LS-DYNA Theory Manual 
22.14  Material Model 14:  Soil and Crushable Foam With 
Failure 
This material model provides the same stress update as model 5.  However, if pressure 
ever reaches its cutoff value, failure occurs and pressure can never again go negative.  In 
material model 5, the pressure is limited to its cutoff value in tension.
LS-DYNA Theory Manual 
Material Models 
22.15  Material Model 15:  Johnson and Cook Plasticity Model 
Johnson and Cook express the flow stress as 
𝜎𝑦 = (𝐴 + 𝐵𝜀̅p𝑛
)(1 + 𝑐ln𝜀̇∗)(1 − 𝑇∗𝑚),
(22.15.1)
where 𝐴, 𝐵, 𝐶, 𝑛,  and  𝑚 are user defined input constants, and: 
𝜀̇∗ =
= effective plastic strain rate for 𝜀̇0, in units of 
𝜀̅𝑝 = effective plastic strain 
̇𝑝
𝜀̅
𝜀̇0
𝑇∗ =
𝑇 − 𝑇room
𝑇melt − 𝑇room
[time]
Constants for a variety of materials are provided in Johnson and Cook [1983]. 
Due  to  the  nonlinearity  in  the  dependence  of  flow  stress  on  plastic  strain,  an 
accurate  value  of  the  flow  stress  requires  iteration  for  the  increment  in  plastic  strain.  
However, by using a Taylor series expansion with linearization about the current time, 
we can solve for 𝜎𝑦 with sufficient accuracy to avoid iteration. 
The strain at fracture is given by 
𝜀f = [𝐷1 + 𝐷2exp (𝐷3𝜎 ∗)][1 + 𝐷4ln𝜀∗][1 + 𝐷5𝑇∗],
(22.15.2)
where  𝐷𝑖, 𝑖 = 1, . . . ,5  are  input  constants  and  𝜎 ∗  is  the  ratio  of  pressure  divided  by 
effective stress: 
𝜎 ∗ =
𝜎eff
.
Fracture occurs when the damage parameter 
𝐷 = ∑
Δ𝜀̅p
𝜀f
reaches the value 1. 
(22.15.3)
(22.15.4)
A choice of three spall models is offered to represent material splitting, cracking, 
and  failure  under  tensile  loads.    The  pressure  limit  model  limits  the  minimum 
hydrostatic pressure to the specified value, 𝑝 ≥ 𝑝min.  If pressures more tensile than this 
limit are calculated, the pressure is reset to 𝑝min.  This option is not strictly a spall model 
since  the  deviatoric  stresses  are  unaffected  by  the  pressure  reaching  the  tensile  cutoff 
and  the  pressure  cutoff  value  𝑝min  remains  unchanged  throughout  the  analysis.    The 
maximum  principal  stress  spall  model  detects  spall  if  the  maximum  principal  stress, 
𝜎max,  exceeds  the  limiting  value  𝜎p.    Once  spall  is  detected  with  this  model,  the 
deviatoric  stresses  are  reset  to  zero  and  no  hydrostatic  tension  is  permitted.    If  tensile
Material Models 
LS-DYNA Theory Manual 
pressures  are  calculated,  they  are  reset  to  0  in  the  spalled  material.    Thus,  the  spalled 
material  behaves  as  rubble.    The  hydrostatic  tension  spall  model  detects  spall  if  the 
pressure becomes more tensile than the specified limit, 𝑝min.  Once spall is detected, the 
deviatoric  stresses  are  set  to  zero  and  the  pressure  is  required  to  be  compressive.    If 
hydrostatic tension is calculated then the pressure is reset to 0 for that element. 
In  addition  to  the  above  failure  criterion,  this  material  model  also  supports  a 
shell  element  deletion  criterion  based  on  the  maximum  stable  time  step  size  for  the 
element,  Δ𝑡max.    Generally,  Δ𝑡max  goes  down  as  the  element  becomes  more  distorted.  
To assure stability of time integration, the global LS-DYNA time step is the minimum of 
the Δ𝑡max values calculated for all elements in the model.  Using this option allows the 
selective  deletion  of  elements  whose  time  step  Δ𝑡max  has  fallen  below  the  specified 
minimum  time  step,  Δ𝑡crit.    Elements  which  are  severely  distorted  often  indicate  that 
material  has  failed  and  supports  little  load,  but  these  same  elements  may  have  very 
small time steps and therefore control the cost of the analysis.  This option allows these 
highly distorted elements to be deleted from the calculation, and, therefore, the analysis 
can proceed at a larger time step, and, thus, at a reduced cost.  Deleted elements do not 
carry  any  load,  and  are  deleted  from  all  applicable  slide  surface  definitions.    Clearly, 
this option must be judiciously used to obtain accurate results at a minimum cost. 
Material  type  15  is  applicable  to  the  high  rate  deformation  of  many  materials 
including  most  metals.    Unlike  the  Steinberg-Guinan  model,  the  Johnson-Cook  model 
remains valid down to lower strain rates and even into the quasistatic regime.  Typical 
applications include explosive metal forming, ballistic penetration, and impact.
LS-DYNA Theory Manual 
Material Models 
22.16  Material Model 16:  Pseudo Tensor 
This  model  can  be  used  in  two  major  modes  -  a  simple  tabular  pressure-
dependent  yield  surface,  and  a  potentially  complex  model  featuring  two  yield  versus 
pressure functions with the means of migrating from one curve to the other.  For both 
modes, load curve N1 is taken to be a strain rate multiplier for the yield strength.  Note 
that this model must be used with equation-of-state type 8 or 9. 
Response Mode I.  Tabulated Yield Stress Versus Pressure 
This  model  is  well  suited  for  implementing  standard  geologic  models  like  the 
Mohr-Coulomb yield surface with a Tresca limit, as shown in Figure 22.16.1.  Examples 
of converting conventional triaxial compression data to this type of model are found in 
(Desai  and  Siriwardane,  1984).    Note  that  under  conventional  triaxial  compression 
conditions,  the  LS-DYNA  input  corresponds  to  an  ordinate  of  𝜎1 − 𝜎3  rather  than  the 
more  widely  used 
,  where  𝜎1  is  the  maximum  principal  stress  and  𝜎3  is  the 
minimum principal stress. 
𝜎1−𝜎3
This  material  combined  with  equation-of-state  type  9  (saturated)  has  been  used 
very  successfully  to  model  ground  shocks  and  soil-structure  interactions  at  pressures 
up to 100kbar. 
To invoke Mode I of this model, set 𝑎0, 𝑎1, 𝑎2, 𝑎0f, and 𝑎1f to zero, The tabulated 
Mohr-Coulomb
Tresca
Friction Angle
Cohesion
Figure 22.16.1.  Mohr-Coulomb surface with a Tresca limit.
Material Models 
LS-DYNA Theory Manual 
values  of  pressure  should  then  be  specified  on  cards  4  and  5,  and  the  corresponding 
values of yield stress should be specified on cards 6 and 7.  The parameters relating to 
reinforcement properties, initial yield stress, and tangent modulus are not used in this 
response mode, and should be set to zero. 
Simple tensile failure 
Note that a1f is reset internally to 1/3 even though it is input as zero; this defines 
a material failure curve of slope 3𝑝, where p denotes pressure (positive in compression).  
In this case the yield strength is taken from the tabulated yield vs.  pressure curve until 
the maximum principal stress (𝜎1) in the element exceeds the tensile cut-off (𝜎cut).  For 
every  time  step  that  𝜎1 > 𝜎cut  the  yield  strength  is  scaled  back  by  a  fraction  of  the 
distance between the two curves until after 20 time steps the yield strength is defined by 
the failure curve.  The only way to inhibit this feature is to set σcut arbitrarily large. 
Response Mode II.  Two-Curve Model with Damage and Failure 
This approach uses two yield versus pressure curves of the form  
𝜎y = 𝑎0 +
𝑎1 + 𝑎2𝑝
.
(22.16.1)
The upper curve is best described as the maximum yield strength curve and the 
lower  curve  is  the  material  failure  curve.    There  are  a  variety  of  ways  of  moving 
between the two curves and each is discussed below. 
MODE II.A: Simple tensile failure 
Define 𝑎0, 𝑎1, 𝑎2, 𝑎0f and 𝑎1f, set 𝑏1 to zero, and leave cards 4 through 7 blank.  In 
this case the yield strength is taken from the maximum yield curve until the maximum 
principal  stress  (𝜎1)  in  the  element  exceeds  the  tensile  cut-off  (𝜎cut).    For  every  time 
Figure 22.2.  Two-curve concrete model with damage and failure. 
Pressure
LS-DYNA Theory Manual 
Material Models 
step that 𝜎1 > 𝜎cut the yield strength is scaled back by a fraction of the distance between 
the two curves until after 20 time steps the yield strength is defined by the failure curve. 
Mode II.B: Tensile failure plus plastic strain scaling 
Define 𝑎0, 𝑎1, 𝑎2, 𝑎0f and 𝑎1f, set 𝑏1 to zero, and user cards 4 through 7 to define a 
scale  factor,  η,  versus  effective  plastic  strain.    LS-DYNA  evaluates  η  at  the  current 
effective plastic strain and then calculated the yield stress as 
𝜎yield = 𝜎failed + 𝜂(𝜎max − 𝜎failed),
(22.16.2)
where 𝜎max and 𝜎failed are found as shown in Figure 19.16.2.  This yield strength is then 
subject to scaling for tensile failure as described above.  This type of model allows the 
description of a strain hardening or softening material such as concrete. 
Mode II.C: Tensile failure plus damage scaling 
The change in yield stress as a function of plastic strain arises from the physical 
mechanisms such as internal cracking, and the extent of this cracking is affected by the 
hydrostatic  pressure  when  the  cracking  occurs.    This  mechanism  gives  rise  to  the 
"confinement" effect on concrete behavior.  To account for this phenomenon, a "damage" 
function was defined and incorporated.  This damage function is given the form: 
𝜀p
𝜆 = ∫ (1 +
𝜎cut
−𝑏1
)
𝑑𝜀p
.
(22.16.3)
Define 𝑎0, 𝑎1, 𝑎2, 𝑎0f and 𝑎1f, and 𝑏1.  Cards 4 through 7 now give 𝜂 as a function 
of 𝜆 and scale the yield stress as 
𝜎yield = 𝜎failed + 𝜂(𝜎max − 𝜎failed),
(22.16.4)
and then apply any tensile failure criteria. 
Mode II Concrete Model Options 
Material Type 16 Mode II provides the option of automatic internal generation of 
a simple "generic" model for concrete.  If 𝑎0 is negative, then 𝜎cut is assumed to be the 
′  and  −𝑎0  is  assumed  to  be  a  conversion 
unconfined  concrete  compressive  strength,  𝑓c
factor from LS-DYNA pressure units to psi.  (For example, if the model stress units are 
MPa, 𝑎0 should be set to –145.) In this case the parameter values generated internally are
Material Models 
LS-DYNA Theory Manual 
(22.16.5) 
𝜎cut = 1.7
′2
⎜⎛ 𝑓c
⎟⎞
−𝑎0⎠
⎝
𝑎0 =
𝑎1 =
′
𝑓c
′ 
3𝑓c
𝑎0f = 0 
𝑎1f = 0.385 
𝑎2 =
Note  that  these  𝑎0f  and  𝑎1f  defaults  will  be  overwritten  by  non-zero  entries  on 
Card 3.  If plastic strain or damage scaling is desired, Cards 5 through 8 and b1 should 
be specified in the input.  When 𝑎0 is input as a negative quantity, the equation-of-state 
can  be  given  as  0  and  a  trilinear  EOS  Type  8  model  will  be  automatically  generated 
from  the  unconfined  compressive  strength  and  Poisson's  ratio.    The  EOS  8  model  is  a 
simple  pressure  versus  volumetric  strain  model  with  no  internal  energy  terms,  and 
should give reasonable results for pressures up to 5kbar (approximately 72,500 psi). 
Mixture model 
A  reinforcement  fraction,  𝑓r,  can  be  defined  along  with  properties  of  the 
reinforcing  material.    The  bulk  modulus,  shear  modulus,  and  yield  strength  are  then 
calculated from a simple mixture rule, i.e., for the bulk modulus the rule gives: 
𝐾 = (1 − 𝑓r)𝐾m + 𝑓r𝐾r,
(22.16.6)
where  𝐾m  and  𝐾r  are  the  bulk  moduli  for  the  geologic  material  and  the  reinforcing 
material, respectively.  This  feature should be used with  caution.  It gives an isotropic 
effect  in  the  material  instead  of  the  true  anisotropic  material  behavior.    A  reasonable 
approach would be to use the mixture elements only where reinforcing material exists 
and  plain  elements  elsewhere.    When  the  mixture  model  is  being  used,  the  strain  rate 
multiplier for the principal material is taken from load curve N1 and the multiplier for 
the reinforcement is taken from load curve N2.
LS-DYNA Theory Manual 
Material Models 
22.17  Material Model 17:  Isotropic Elastic-Plastic With 
Oriented Cracks 
This is an isotropic elastic-plastic material which includes a failure model with an 
oriented crack.  The von Mises yield condition is given by: 
𝜎y
where  the  second  stress  invariant,  𝐽2,  is  defined  in  terms  of  the  deviatoric  stress 
components as 
𝜙 = 𝐽2 −
(22.17.1)
,
𝐽2 =
𝑠𝑖𝑗𝑠𝑖𝑗,
(22.17.2)
and the yield stress, 𝜎y,  is a  function of the effective plastic strain,  𝜀eff
hardening modulus, 𝐸p: 
p , and the plastic 
p .
𝜎y = 𝜎0 + 𝐸p𝜀eff
(22.17.3)
The effective plastic strain is defined as: 
p = ∫ 𝑑𝜀eff
𝜀eff
,
(22.17.4)
p = √2
where  𝑑𝜀eff
input tangent modulus, 𝐸t, as 
3 𝑑𝜀𝑖𝑗
p𝑑𝜀𝑖𝑗
p,  and  the  plastic  tangent  modulus  is  defined  in  terms  of  the 
𝐸p =
𝐸𝐸t
𝐸 − 𝐸t
.
(22.17.5)
Pressure in this model is found from evaluating an equation of state.  A pressure 
cutoff can be defined such that the pressure is not allowed to fall below the cutoff value. 
The  oriented  crack  fracture  model  is  based  on  a  maximum  principal  stress 
criterion.    When  the  maximum  principal  stress  exceeds  the  fracture  stress,  𝜎f,  the 
element fails on a plane perpendicular to the direction of the maximum principal stress.  
The  normal  stress  and  the  two  shear  stresses  on  that  plane  are  then  reduced  to  zero.  
This  stress  reduction  is  done  according  to  a  delay  function  that  reduces  the  stresses 
gradually to zero over a small number of time steps.  This delay function procedure is 
used  to  reduce  the  ringing  that  may  otherwise  be  introduced  into  the  system  by  the 
sudden fracture.
Material Models 
LS-DYNA Theory Manual 
After a tensile fracture, the element will not support tensile stress on the fracture 
plane, but in compression will support both normal and shear stresses.  The orientation 
of  this  fracture  surface  is  tracked  throughout  the  deformation,  and  is  updated  to 
  If  the  maximum  principal  stress 
properly  model  finite  deformation  effects. 
subsequently  exceeds  the  fracture  stress  in  another  direction,  the  element  fails 
isotropically.  In this case the element completely loses its ability to support any shear 
stress  or  hydrostatic  tension,  and  only  compressive  hydrostatic  stress  states  are 
possible.  Thus, once isotropic failure has occurred, the material behaves like a fluid. 
This  model  is  applicable  to  elastic  or  elastoplastic  materials  under  significant 
tensile or shear loading when fracture is expected.  Potential applications include brittle 
materials such as ceramics as well as porous materials such as concrete in cases where 
pressure hardening effects are not significant.
LS-DYNA Theory Manual 
Material Models 
22.18  Material Model 18:  Power Law Isotropic Plasticity 
Elastoplastic behavior with isotropic hardening is provided by this model.  The 
yield stress, 𝜎y, is a function of plastic strain and obeys the equation: 
𝜎y = 𝑘𝜀𝑛 = 𝑘(𝜀yp + 𝜀̅p)
,
(22.18.1)
where 𝜀yp is the elastic strain to yield and 𝜀̅p is the effective plastic strain (logarithmic).   
A parameter, SIGY, in the input governs how the strain to yield is identified.  If 
SIGY  is  set  to  zero,  the  strain  to  yield  if  found  by  solving  for  the  intersection  of  the 
linearly elastic loading equation with the strain hardening equation: 
which gives the elastic strain at yield as: 
𝜎 = 𝐸𝜀,
𝜎 = 𝑘𝜀𝑛,
𝜀yp = (
𝑛−1
.
)
If SIGY yield is nonzero and greater than 0.02 then: 
𝜀yp = (
𝜎y
.
)
(22.18.2)
(22.18.3)
(22.18.4)
Strain  rate  is  accounted  for  using the  Cowper-Symonds  model  which  scales  the 
yield stress with the factor 
1 + (
P⁄
)
,
𝜀̇
(22.18.5)
where 𝜀̇ is the strain rate.  A fully viscoplastic formulation is optional with this model 
which  incorporates  the  Cowper-Symonds  formulation  within  the  yield  surface.    An 
additional cost is incurred but the improvement allows for dramatic results.
Material Models 
LS-DYNA Theory Manual 
22.19  Material Model 19:  Strain Rate Dependent Isotropic 
Plasticity 
In this model, a load curve is used to describe the yield strength 𝜎0 as a function 
of effective strain rate 𝜀̅
̇ where 
𝜀̅
̇  = (
2⁄
′ )
′ 𝜀̇𝑖𝑗
𝜀̇𝑖𝑗
,
(22.19.1)
and the prime denotes the deviatoric component.  The yield stress is defined as 
̇ ) + 𝐸p𝜀̅p.
(22.19.2)
where 𝜀̅p is the effective plastic strain and 𝐸p is given in terms of Young’s modulus and 
the tangent modulus by 
𝜎y = 𝜎0(𝜀̅
𝐸p =
𝐸𝐸t
𝐸 − 𝐸t
.
(22.19.3)
Both  Young's  modulus  and  the  tangent  modulus  may  optionally  be  made 
functions of strain rate by specifying a load curve ID giving their values as a function of 
strain rate.  If these load curve ID's are input as 0, then the constant values specified in 
the input are used. 
Note  that  all  load  curves  used  to  define  quantities  as  a  function  of  strain  rate 
must have the same number of points at the same strain rate values.  This requirement 
is  used  to  allow  vectorized  interpolation  to  enhance  the  execution  speed  of  this 
constitutive model. 
This model also contains a simple mechanism for modeling material failure.  This 
option is activated by specifying a load curve ID defining the effective stress at failure 
as  a  function  of  strain  rate.    For  solid  elements,  once  the  effective  stress  exceeds  the 
failure  stress  the  element  is  deemed  to  have  failed  and  is  removed  from  the  solution.  
For  shell  elements  the  entire  shell  element  is  deemed  to  have  failed  if  all  integration 
points  through  the  thickness  have  an  effective  stress  that  exceeds  the  failure  stress.  
After failure the shell element is removed from the solution. 
In  addition  to  the  above  failure  criterion,  this  material  model  also  supports  a 
shell  element  deletion  criterion  based  on  the  maximum  stable  time  step  size  for  the 
element,  Δ𝑡max.    Generally,  Δ𝑡max  goes  down  as  the  element  becomes  more  distorted.  
To assure stability of time integration, the global LS-DYNA time step is the minimum of 
the Δ𝑡max values calculated for all elements in the model.  Using this option allows the 
selective  deletion  of  elements  whose  time  step  Δ𝑡max  has  fallen  below  the  specified 
minimum  time  step,  Δ𝑡crit.    Elements  which  are  severely  distorted  often  indicate  that
LS-DYNA Theory Manual 
Material Models 
material  has  failed  and  supports  little  load,  but  these  same  elements  may  have  very 
small time steps and therefore control the cost of the analysis.  This option allows these 
highly distorted elements to be deleted from the calculation, and, therefore, the analysis 
can proceed at a larger time step, and, thus, at a reduced cost.  Deleted elements do not 
carry  any  load,  and  are  deleted  from  all  applicable  slide  surface  definitions.    Clearly, 
this option must be judiciously used to obtain accurate results at a minimum cost.
Material Models 
LS-DYNA Theory Manual 
22.20  Material Model 20:  Rigid 
The  rigid  material  type  20  provides  a  convenient  way  of  turning  one  or  more 
parts comprised of beams, shells, or solid elements into a rigid body.  Approximating a 
deformable  body  as  rigid  is  a  preferred  modeling  technique  in  many  real  world 
applications.    For  example,  in  sheet  metal  forming  problems  the  tooling  can  properly 
and accurately be treated as rigid.  In the design of restraint systems the occupant can, 
for  the  purposes  of  early  design  studies,  also  be  treated  as  rigid.    Elements  which  are 
rigid  are  bypassed  in  the  element  processing  and  no  storage  is  allocated  for  storing 
history variables; consequently, the rigid material type is very cost efficient. 
Two unique rigid part IDs may not share common nodes unless they are merged 
together using the rigid body merge option.  A rigid body may be made up of disjoint 
finite  element  meshes,  however.    LS-DYNA  assumes  this  is  the  case  since  this  is  a 
common practice in setting up tooling meshes in forming problems. 
All elements which reference a given part ID corresponding to the rigid material 
should be contiguous, but this is not a requirement.  If two disjoint groups of elements 
on opposite sides of a model are modeled as rigid, separate part ID's should be created 
for each of the contiguous element groups if each group is to move independently.  This 
requirement arises from the fact that LS-DYNA internally computes the six rigid body 
degrees-of-freedom for each rigid body (rigid material or set of merged materials), and 
if disjoint groups of rigid elements use the same part ID, the disjoint groups will move 
together as one rigid body.   
Inertial properties for rigid materials may be defined in either of two ways.  By 
default,  the  inertial  properties  are  calculated  from  the  geometry  of  the  constituent 
elements of the rigid material and the density specified for the part ID.  Alternatively, 
the inertial properties and initial velocities for a rigid body may be directly defined, and 
this  overrides  data  calculated  from  the  material  property  definition  and  nodal  initial 
velocity definitions. 
Young's  modulus,  E,  and  Poisson's  ratio,  υ  are  used  for  determining  sliding 
interface parameters if the rigid body interacts in a contact definition.  Realistic values 
for  these  constants  should  be  defined  since  unrealistic  values  may  contribute  to 
numerical problem in contact.
LS-DYNA Theory Manual 
Material Models 
22.21  Material Model 21:  Thermal Orthotropic Elastic 
In  the  implementation  for  three-dimensional  continua  a  total  Lagrangian 
formulation  is  used.    In  this  approach  the  material  law  that  relates  second  Piola-
Kirchhoff stress 𝐒 to the Green-St.  Venant strain 𝐄 is 
𝐒 = 𝐂 ⋅ 𝐄 = 𝐓T𝐂l𝐓 ⋅ 𝐄,
where 𝐓 is the transformation matrix [Cook 1974]. 
𝐓 =
𝑙1
⎡
⎢
𝑙2
⎢
⎢
𝑙3
⎢
⎢
2𝑙1𝑙2
⎢
2𝑙2𝑙3
⎢
2𝑙3𝑙1
⎣
𝑚1
𝑚2
𝑚3
2𝑚1𝑚2
2𝑚2𝑚3
2𝑚3𝑚1
𝑛1
𝑛2
𝑛3
2𝑛1𝑛2
2𝑛2𝑛3
2𝑛3𝑛1
𝑙1𝑚1
𝑙2𝑚2
𝑙3𝑚3
(𝑙1𝑚2 + 𝑙2𝑚1)
(𝑙2𝑚3 + 𝑙3𝑚2)
(𝑙3𝑚1 + 𝑙1𝑚3)
𝑚1𝑛1
𝑚2𝑛2
𝑚3𝑛3
(𝑚1𝑛2 + 𝑚2𝑛1)
(𝑚2𝑛3 + 𝑚3𝑛2)
(𝑚3𝑛1 + 𝑚1𝑛3)
𝑛1𝑙1
⎤
⎥
𝑛2𝑙2
⎥
⎥
𝑛3𝑙3
, 
⎥
⎥
(𝑛1𝑙2 + 𝑛2𝑙1)
⎥
(𝑛2𝑙3 + 𝑛3𝑙2)
⎥
(𝑛3𝑙1 + 𝑛1𝑙3)⎦
𝑙𝑖, 𝑚𝑖, 𝑛𝑖 are the direction cosines 
(22.21.1)
(22.21.2)
(22.21.3)
′ denotes the material axes.  The constitutive matrix 𝐂l is defined in terms of the 
′ = 𝑙𝑖𝑥1 + 𝑚𝑖𝑥2 + 𝑛𝑖𝑥3       for  𝑖 = 1, 2, 3,
𝑥𝑖
and 𝑥𝑖
material axes as 
−1 =
𝐂l
𝐸11
𝜐12
𝐸 11
𝜐13
𝐸11
−
−
−
−
𝜐21
𝐸22
𝐸22
𝜐23
𝐸22
−
−
𝜐31
𝐸33
𝜐32
𝐸33
𝐸33
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
𝐺12
𝐺23
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
, 
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
𝐺31⎦
(22.21.4)
where the subscripts denote the material axes, i.e., 
υ𝑖𝑗 = υ𝑥′𝑖 𝑥′𝑗
and 𝐸𝑖𝑖 = 𝐸𝑥′𝑖.
(22.21.5)
Since 𝐂l is symmetric 
υ12
𝐸11
=
υ21
𝐸22
, etc.
(22.21.6)
Material Models 
LS-DYNA Theory Manual 
The vector of Green-St.  Venant strain components is 
𝐄T = [𝐸11 𝐸22 𝐸33 𝐸12 𝐸23 𝐸31],
which include the local thermal strains which are integrated in time: 
𝑛+1 = 𝜀𝑎𝑎
𝜀𝑎𝑎
𝑛+1 = 𝜀𝑏𝑏
𝜀𝑏𝑏
𝑛+1 = 𝜀𝑐𝑐
𝜀𝑐𝑐
𝑛 + 𝛼𝑎(𝑇𝑛+1 − 𝑇𝑛),
𝑛 + 𝛼𝑏(𝑇𝑛+1 − 𝑇𝑛), 
𝑛 + 𝛼𝑐(𝑇𝑛+1 − 𝑇𝑛).
(22.21.7)
(22.21.8)
After  computing  𝑆𝑖𝑗  we  use  Equation  (18.32)  to  obtain  the  Cauchy  stress.    This 
model will predict realistic behavior for finite displacement and rotations as long as the 
strains are small. 
For  shell  elements,  the  stresses  are  integrated  in  time  and  are  updated  in  the 
corotational coordinate system.  In this procedure the local material axes are assumed to 
remain  orthogonal  in  the  deformed  configuration.    This  assumption  is  valid  if  the 
strains remain small.
LS-DYNA Theory Manual 
Material Models 
22.22  Material Model 22:  Chang-Chang Composite Failure 
Model 
For  shells,  five  material  parameters  are  used  in  the  three  failure  criteria.    These 
are [Chang and Chang 1987a, 1987b]: 
•  𝑆1, longitudinal tensile strength 
•  𝑆2, transverse tensile strength 
•  𝑆12, shear strength 
•  𝐶2, transverse compressive strength 
•  𝛼, nonlinear shear stress parameter. 
𝑆1,  𝑆2,  𝑆12,  and  𝐶2  are  obtained  from  material  strength  measurement.    𝛼  is  defined  by 
material shear stress-strain measurements.  In plane stress, the strain is given in terms 
of the stress as 
(𝜎1 − 𝜐1𝜎2),
(𝜎2 − 𝜐2𝜎1), 
(22.22.1)
𝜀1 =
𝜀2 =
𝐸1
𝐸2
2𝜀12 =
3 .
𝜏12 + 𝛼𝜏12
𝐺12
The third equation defines the nonlinear shear stress parameter 𝛼.  A fiber matrix 
shearing term augments each damage mode: 
𝜏̅ =
𝜏12
2𝐺12
𝑆12
2𝐺12
+ 3
+ 3
𝛼𝜏12
𝛼𝑆12
, 
which is the ratio of the shear stress to the shear strength. 
The matrix cracking failure criteria is determined from 
𝐹matrix = (
)
𝜎2
𝑆2
+ 𝜏̅,
(22.22.2)
(22.22.3)
where  failure  is  assumed  whenever  𝐹matrix > 1.    If  𝐹matrix > 1,  then  the  material 
constants 𝐸2, 𝐺12, 𝜐1, and 𝜐2 are set to zero. 
The compression failure criteria is given as
Material Models 
LS-DYNA Theory Manual 
𝐹comp = (
𝜎2
2𝑆12
)
+
)
𝐶2
2𝑆12
⎢⎡(
⎣
− 1
⎥⎤ 𝜎2
𝐶2
⎦
+ 𝜏̅,
(22.22.4)
where failure is assumed whenever 𝐹comb > 1.  If 𝐹comb > 1, then the material constants 
𝐸2, 𝜐1, and 𝜐2 are set to zero. 
The final failure mode is due to fiber breakage. 
𝐹fiber = (
)
𝜎1
S1
+ 𝜏̅,
(22.22.5)
Failure  is  assumed  whenever 𝐹fiber > 1.    If  𝐹fiber > 1,  then  the constants  𝐸1,  𝐸2,  𝐺12  𝜐1 
and 𝜐2 are set to zero. 
For solids, a fourth failure mode corresponding to delamination is computed as    
𝐹delam = (
max (0.0, 𝜎3)
S3
)
+ (
)
𝜏23
S23
+ (
)
𝜏31
S31
This involves three additional material parameters. 
•  𝑆3, normal tensile strength 
•  𝑆23, transverse shear strength 
•  𝑆31, transverse shear strength 
(22.22.140)
LS-DYNA Theory Manual 
Material Models 
22.23  Material Model 23:  Thermal Orthotropic Elastic with 
12 Curves 
In  the  implementation  for  three-dimensional  continua  a  total  Lagrangian 
formulation  is  used.    In  this  approach  the  material  law  that  relates  second  Piola-
Kirchhoff stress 𝐒 to the Green-St.  Venant strain 𝐄 is 
𝐒 = 𝐂 ⋅ 𝐄 = 𝐓T𝐂l𝐓 ⋅ 𝐄,
where 𝐓 is the transformation matrix [Cook 1974]. 
𝐓 =
𝑙1
⎡
⎢
𝑙2
⎢
⎢
𝑙3
⎢
⎢
2𝑙1𝑙2
⎢
2𝑙2𝑙3
⎢
2𝑙3𝑙1
⎣
𝑚1
𝑚2
𝑚3
2𝑚1𝑚2
2𝑚2𝑚3
2𝑚3𝑚1
𝑙𝑖, 𝑚𝑖, 𝑛𝑖 are the direction cosines 
𝑛1
𝑛2
𝑛3
2𝑛1𝑛2
2𝑛2𝑛3
2𝑛3𝑛1
𝑙1𝑚1
𝑙2𝑚2
𝑙3𝑚3
(𝑙1𝑚2 + 𝑙1𝑚1)
(𝑙2𝑚3 + 𝑙3𝑚2)
(𝑙3𝑚1 + 𝑙1𝑚3)
𝑚1𝑛1
𝑚2𝑛2
𝑚3𝑛3
(𝑚1𝑛2 + 𝑚2𝑛1)
(𝑚2𝑛3 + 𝑚3𝑛2)
(𝑚3𝑛1 + 𝑚1𝑛3)
𝑛1𝑙1
⎤
⎥
𝑛2𝑙2
⎥
⎥
𝑛3𝑙3
⎥
⎥
(𝑛1𝑙2 + 𝑛2𝑙1)
⎥
(𝑛2𝑙3 + 𝑛3𝑙2)
⎥
(𝑛3𝑙1 + 𝑛1𝑙3)⎦
, 
(22.23.1)
(22.23.2)
(22.23.3)
′ denotes the material axes.  The temperature dependent constitutive matrix 𝐂l is 
′ = 𝑙𝑖𝑥1 + 𝑚𝑖𝑥2 + 𝑛𝑖𝑥3
𝑥𝑖
for 𝑖 = 1, 2, 3,
and 𝑥𝑖
defined in terms of the material axes as 
−1 =
𝐂l
𝐸11(𝑇)
𝜐12(𝑇)
𝐸11(𝑇)
𝜐13(𝑇)
𝐸11(𝑇)
−
−
−
−
𝜐21(𝑇)
𝐸22(𝑇)
𝐸22(𝑇)
𝜐23(𝑇)
𝐸 22(𝑇)
−
−
𝜐31(𝑇)
𝐸33(𝑇)
𝜐32(𝑇)
𝐸33(𝑇)
𝐸33(𝑇)
⎡
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣
𝐺12(𝑇)
𝐺23(𝑇)
⎤
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
, 
⎥
⎥
⎥
⎥
⎥
⎥
⎥
⎥
𝐺31(𝑇)⎦
(22.23.4)
where the subscripts denote the material axes, i.e., 
𝜐𝑖𝑗 = υ𝑥′𝑖 𝑥′𝑗
and 𝐸𝑖𝑖 = 𝐸𝑥′𝑖.
(22.23.5)
Since 𝐂l is symmetric 
𝜐12
𝐸11
=
𝜐21
𝐸22
, etc.
(22.23.6)
Material Models 
LS-DYNA Theory Manual 
The vector of Green-St.  Venant strain components is 
𝐄T = [𝐸11 𝐸22 𝐸33 𝐸12 𝐸23 𝐸31],
which include the local thermal strains which are integrated in time: 
𝑛+1 = 𝜀𝑎𝑎
𝜀𝑎𝑎
𝑛 + 𝛼𝑎 (𝑇
𝑛+1
2) [𝑇𝑛+1 − 𝑇𝑛],
𝑛+1 = 𝜀𝑏𝑏
𝜀𝑏𝑏
𝑛 + 𝛼𝑏 (𝑇
𝑛+1
2) [𝑇𝑛+1 − 𝑇𝑛], 
𝑛+1 = 𝜀𝑐𝑐
𝜀𝑐𝑐
𝑛 + 𝛼𝑐 (𝑇
𝑛+1
2) [𝑇𝑛+1 − 𝑇𝑛].
(22.23.7)
(22.23.8)
After  computing  𝑆𝑖𝑗  we  use  Equation  (16.32)  to  obtain  the  Cauchy  stress.    This 
model will predict realistic behavior for finite displacement and rotations as long as the 
strains are small. 
For  shell  elements,  the  stresses  are  integrated  in  time  and  are  updated  in  the 
corotational coordinate system.  In this procedure the local material axes are assumed to 
remain  orthogonal  in  the  deformed  configuration.    This  assumption  is  valid  if  the 
strains remain small.
LS-DYNA Theory Manual 
Material Models 
22.24  Material Model 24:  Piecewise Linear Isotropic 
Plasticity 
This plasticity treatment in this model is quite similar to Model 10, but unlike 10, 
it includes strain rate effects and does not use an equation of state.  Deviatoric stresses 
are determined that satisfy the yield function 
𝜙 =
𝑠𝑖𝑗𝑠𝑖𝑗 −
𝜎y
≤ 0,
(22.24.1)
where 
where  the  hardening  function  𝑓h(𝜀eff
Otherwise, linear hardening of the form 
σy = 𝛽[𝜎0 + 𝑓h(𝜀eff
(22.24.2)
p )  can  be  specified  in  tabular  form  as  an  option.  
p )],
p ) = 𝐸p(𝜀eff
p ),
𝑓h(𝜀eff
(22.24.3)
p   are  given  in  Equations  (22.3.6)  and  (8.61),  respectively.  
is  assumed  where  𝐸p  and  𝜀eff
The  parameter  𝛽  accounts  for  strain  rate  effects.    For  complete  generality  a  table 
defining  the  yield  stress  versus  plastic  strain  may  be  defined  for  various  levels  of 
effective strain rate. 
In the implementation of this material model, the deviatoric stresses are updated 
elastically , the yield function is checked, and if it is satisfied the 
deviatoric stresses are accepted.  If it is not, an increment in plastic strain is computed: 
p =
Δ𝜀eff
(3
2⁄
∗ )
∗ 𝑠𝑖𝑗
𝑠𝑖𝑗
3𝐺 + 𝐸p
− 𝜎y
,
(22.24.4)
is  the  shear  modulus  and  𝐸p  is  the  current  plastic  hardening  modulus.    The  trial 
deviatoric stress state 𝑠𝑖𝑗
∗  is scaled back: 
𝑛+1 =
𝑠𝑖𝑗
𝜎𝑦
2⁄
∗ )
∗ 𝑠𝑖𝑗
𝑠𝑖𝑗
(3
∗ .
𝑠𝑖𝑗
(22.24.5)
For  shell  elements,  the  above  equations  apply,  but  with  the  addition  of  an 
iterative loop to solve for the normal strain increment, such that the stress component 
normal to the mid surface of the shell element approaches zero. 
Three options to account for strain rate effects are possible:
Material Models 
LS-DYNA Theory Manual 
1. 
Strain  rate  may  be  accounted  for  using  the  Cowper-Symonds  model  which 
scales the yield stress with the factor 
𝛽 = 1 + (
𝑝⁄
)
.
𝜀̇
(22.24.6)
where 𝜀̇ is the strain rate. 
2. 
3. 
For complete generality a load curve, defining 𝛽, which scales the yield stress 
may  be  input  instead.    In  this  curve  the  scale  factor  versus  strain  rate  is  de-
fined. 
If different stress versus strain curves can be provided for various strain rates, 
the  option  using  the  reference  to  a  table  definition  can  be  used.    See  Fig-
ure 19.24.1. 
A  fully  viscoplastic  formulation  is  optional  which  incorporates  the  different 
options above within the yield surface.  An additional cost is incurred over the simple 
scaling but the improvement is results can be dramatic. 
If  a  table  ID  is  specified  a  curve  ID  is  given  for  each  strain  rate,  see  Section  23.  
Intermediate values are found by interpolating between curves.  Effective plastic strain 
versus yield stress is expected.  If the strain rate values fall out of range, extrapolation is 
not used; rather, either the first or last curve determines the yield stress depending on 
whether the rate is low or high, respectively.
LS-DYNA Theory Manual 
Material Models 
22.25  Material Model 25:  Kinematic Hardening Cap Model 
The  implementation  of  an  extended  two  invariant  cap  model,  suggested  by 
Stojko [1990], is based on the formulations of Simo, et al.  [1988, 1990] and Sandler and 
Rubin  [1979].    In  this  model,  the  two  invariant  cap  theory  is  extended  to  include 
nonlinear  kinematic  hardening as  suggested  by  Isenberg,  Vaughn,  and  Sandler  [1978].  
A brief discussion of the extended cap model and its parameters is given below. 
The cap model is formulated in terms of the invariants of the stress tensor.  The 
square  root  of  the  second  invariant  of  the  deviatoric  stress  tensor,  √𝐽2D  is  found  from 
the deviatoric stresses 𝐒 as 
√𝐽2D ≡ √
𝑠𝑖𝑗𝑠𝑖𝑗,
(22.25.1)
and  is  the  objective  scalar  measure  of  the  distortional  or  shearing  stress.    The  first 
invariant of the stress, 𝐽1, is the trace of the stress tensor. 
The  cap  model  consists  of  three  surfaces  in √𝐽2D − 𝐽1 space,  as  shown  in  Figure 
22.25.1.  First, there is a failure envelope surface, denoted 𝑓1 in the figure.  The functional 
form of 𝑓1 is 
where 𝐹e is given by 
𝑓1 = √𝐽2D − min(𝐹e(𝐽1), 𝑇mises),
𝐹e(𝐽1) ≡ 𝛼 − 𝛾exp(−𝛽𝐽1) + 𝜃𝐽1.
(22.25.2)
(22.25.3)
εp
eff
Figure  22.25.1.    Rate  effects  may  be  accounted  for  by  defining  a  table  of
curves.
Material Models 
LS-DYNA Theory Manual 
2D
J = Fe
2D
f1
f3
J = Fc
2D
f2
J1
X( )
Figure  22.25.2.    The  yield  surface  of  the  two-invariant  cap  model  in 
pressure √𝐽2D − 𝐽1 space Surface 𝑓1 is the failure envelope, 𝑓2 is the cap surface, 
and 𝑓3 is the tension cutoff.   
and  𝑇mises ≡ |𝑋(𝜅𝑛) − 𝐿(𝜅𝑛)|.    This  failure  envelope  surface  is  fixed  in  √𝐽2D − 𝐽1  space, 
and therefore does not harden unless kinematic hardening is present.  Next, there is a 
cap surface, denoted 𝑓2 in the figure, with 𝑓2 given by 
where 𝐹c is defined by 
𝑓2 = √𝐽2D − 𝐹c(𝐽1, 𝜅),
𝑋(𝜅) is the intersection of the cap surface with the 𝐽1 axis 
√[𝑋(𝜅) − 𝐿(𝜅)] 2 − [𝐽1 − 𝐿(𝜅)] 2,
𝐹c(𝐽1, 𝜅) ≡
and 𝐿(𝜅) is defined by  
𝑋(𝜅) = 𝜅 + 𝑅𝐹e(𝜅),
𝐿(𝜅) ≡ {
𝜅 > 0
0 𝜅 ≤ 0
.
(22.25.4)
(22.25.5)
(22.25.6)
(22.25.7)
The hardening parameter 𝜅 is related to the plastic volume change 𝜀v
p through the 
hardening law 
p = W{1 − exp[−𝐷(𝑋(κ) − 𝑋0)]}.
𝜀v
(22.25.8)
Geometrically, 𝜅 is seen in the figure as the 𝐽1 coordinate of the intersection of the 
cap surface and the failure surface.  Finally, there is the tension cutoff surface, denoted 
𝑓3 in the figure.  The function 𝑓3 is given by 
𝑓3 + 𝑇 − 𝐽1,
(22.25.9)
where  𝑇  is  the  input  material  parameter  which  specifies  the  maximum  hydrostatic 
tension  sustainable  by  the  material.    The  elastic  domain  in  √𝐽2D − 𝐽1  space  is  then
LS-DYNA Theory Manual 
Material Models 
bounded  by  the  failure  envelope  surface  above,  the  tension  cutoff  surface  on  the  left, 
and the cap surface on the right. 
An additive decomposition of the strain into elastic and plastic parts is assumed: 
(22.25.10)
where 𝜀e is the elastic strain and 𝜀p is the plastic strain.  Stress is found from the elastic 
strain using Hooke’s law, 
𝜀 = 𝜀 + 𝜀P,
𝜎 = 𝐶(𝜀 − 𝜀P),
(22.25.11)
where 𝜎 is the stress and 𝐶 is the elastic constitutive tensor. 
The yield condition may be written 
𝑓1(𝜎) ≤ 0,
𝑓2(𝜎, 𝜅) ≤ 0, 
𝑓3(𝜎) ≤ 0,
and the plastic consistency condition requires that 
𝜆̇𝑘𝑓𝑘 = 0
𝜆̇𝑘 ≥ 0
𝑘 = 1, 2, 3,
(22.25.12)
(22.25.13)
where 𝜆𝑘 is the plastic consistency parameter for surface 𝑘.  If 𝑓𝑘 < 0, then 𝜆̇𝑘 = 0 and the 
response  is  elastic.    If  𝑓𝑘 > 0,  then  surface  k  is  active  and  𝜆̇𝑘  is  found  from  the 
requirement that 𝑓 ̇
𝑘 = 0. 
Associated plastic flow is assumed, so using Koiter’s flow rule the plastic strain 
rate is given as the sum of contribution from all of the active surfaces, 
𝜀̇p = ∑ 𝜆̇𝑘
𝑘=1
∂𝑓𝑘
∂𝑠
.
(22.25.14)
One  of  the  major  advantages  of  the  cap  model  over  other  classical  pressure-
dependent plasticity models is the ability to control the amount of dilatency produced 
under shear loading.  Dilatency is produced under shear loading as a result of the yield 
surface having a positive slope in √𝐽2D − 𝐽1 space, so the assumption of plastic flow in 
the direction normal to the yield surface produces a plastic strain rate vector that has a 
component  in  the  volumetric  (hydrostatic)  direction  .    In  models 
such  as  the  Drucker-Prager  and  Mohr-Coulomb,  this  dilatency  continues  as  long  as 
shear  loads  are  applied,  and  in  many  cases  produces  far  more  dilatency  than  is 
experimentally observed in material tests.  In the cap model, when the failure surface is 
active,  dilatency  is  produced  just  as  with  the  Drucker-Prager  and  Mohr-Columb 
models.  However, the hardening law permits the cap surface to contract until the cap 
intersects the failure envelope at the stress point, and the cap remains at that point.  The 
local  normal  to  the  yield  surface  is  now  vertical,  and  therefore  the  normality  rule 
assures  that  no  further  plastic  volumetric  strain  (dilatency)  is  created.    Adjustment  of
Material Models 
LS-DYNA Theory Manual 
the  parameters  that  control  the  rate  of  cap  contractions  permits  experimentally 
observed amounts of dilatency to be incorporated into the cap model, thus producing a 
constitutive law which better represents the physics to be modeled.  Another advantage 
of the cap model over other models such as the Drucker-Prager and Mohr-Coulomb is 
the ability to model plastic compaction.  In these models all purely volumetric response 
is elastic.  In the cap model, volumetric response is elastic until the stress point hits the 
cap  surface.    Therefore,  plastic  volumetric  strain  (compaction)  is  generated  at  a  rate 
controlled  by  the  hardening  law.    Thus,  in  addition  to  controlling  the  amount  of 
dilatency,  the  introduction  of  the  cap  surface  adds  another  experimentally  observed 
response characteristic of geological material into the model. 
The  inclusion  of  kinematic  hardening  results  in  hysteretic  energy  dissipation 
under  cyclic  loading  conditions.    Following  the  approach  of  Isenberg,  et  al.,  [1978]  a 
nonlinear  kinematic  hardening  law  is  used  for  the  failure  envelope  surface  when 
nonzero  values  of  and  N  are  specified.    In  this  case,  the  failure  envelope  surface  is 
replaced by a family of yield surfaces bounded by an initial yield surface and a limiting 
failure envelope surface.  Thus, the shape of the yield surfaces described above remains 
unchanged, but they may translate in a plane orthogonal to the J axis. 
Translation of the yield surfaces is permitted through the introduction of a “back 
stress”  tensor,  α.    The  formulation  including  kinematic  hardening  is  obtained  by 
replacing  the  stress  σ  with  the  translated  stress  tensor  𝜂 ≡ 𝜎 − 𝛼  in  all  of  the  above 
equation.  The history tensor α is assumed deviatoric, and therefore has only 5 unique 
components.    The  evolution  of  the  back  stress  tensor  is  governed  by  the  nonlinear 
hardening law 
(22.25.15)
where  c̅  is  a  constant,  𝐹̅  is  a  scalar  function  of  𝜎  and  𝛼  and  𝜀̇p  is  the  rate  of  deviator 
plastic strain.  The constant may be estimated from the slope of the shear stress - plastic 
shear strain curve at low levels of shear stress. 
𝛼 = c̅𝐹̅(𝜎, 𝛼) 𝜀̇p,
The function 𝐹̅ is defined as 
𝐹̅ ≡ max (0,1 −
(𝜎 − 𝛼)𝛼
2N𝐹𝑒(𝐽1)
),
(22.25.16)
where  N  is  a  constant  defining  the  size  of  the  yield  surface.    The  value  of  N  may  be 
interpreted as the radial distant between the outside of the initial yield surface and the 
inside of the limit surface.  In order for the limit surface of the kinematic hardening cap 
model  to  correspond with  the  failure  envelope  surface  of  the  standard  cap  model,  the 
scalar parameter a must be replaced α − N in the definition 𝐹e. 
The  cap  model  contains  a  number  of  parameters  which  must  be  chosen  to 
represent  a  particular  material,  and  are  generally  based  on  experimental  data.    The 
parameters 𝛼,  𝛽,  𝜃  and  𝛾  are  usually  evaluated  by  fitting  a  curve  through  failure  data 
taken from a set of triaxial compression tests.  The parameters 𝑊, 𝐷, and X0 define the
LS-DYNA Theory Manual 
Material Models 
cap  hardening  law.    The  value  W  represents  the  void  fraction  of  the  uncompressed 
sample and 𝐷 governs the slope of the initial loading curve in hydrostatic compression.  
The value of R is the ration of major to minor axes of the quarter ellipse defining the cap 
surface.    Additional  details  and  guidelines  for  fitting  the  cap  model  to  experimental 
data are found in [Chen and Baladi, 1985].
Material Models 
LS-DYNA Theory Manual 
22.26  Material Model 26:  Crushable Foam 
This  orthotropic  material  model  does  the  stress  update  in  the  local  material 
system denoted by the subscripts, 𝑎, 𝑏, and 𝑐.  The material model requires the following 
input parameters: 
•  E, Young’s modulus for the fully compacted material; 
•  𝜈, Poisson’s ratio for the compacted material;  
•  𝜎y, yield stress for fully compacted honeycomb;  
•  LCA, load curve number for sigma-aa versus either relative volume or volumet-
ric strain ; 
•  LCB, load curve number for sigma-bb versus either relative volume or volumet-
ric strain  (default:  LCB = LCA); 
•  LCC,  the  load  curve  number  for  sigma-cc  versus  either  relative  volume  or 
volumetric strain (default: LCC = LCA); 
•  LCS,  the  load  curve  number  for  shear  stress  versus  either  relative  volume  or 
volumetric strain (default LCS = LCA); 
•  𝑉f, relative volume at which the honeycomb is fully compacted;  
•  𝐸𝑎𝑎u, elastic modulus in the uncompressed configuration; 
•  𝐸𝑏𝑏u, elastic modulus in the uncompressed configuration; 
•  𝐸𝑐𝑐u, elastic modulus in the uncompressed configuration; 
•  𝐺𝑎𝑏u, elastic shear modulus in the uncompressed configuration; 
•  𝐺𝑏𝑐u, elastic shear modulus in the uncompressed configuration;  
•  𝐺𝑐𝑎u, elastic shear modulus in the uncompressed configuration; 
•  LCAB,  load  curve  number  for  sigma-ab  versus  either  relative  volume  or 
volumetric strain (default:  LCAB = LCS);  
•  LCBC,  load  curve  number  for  sigma-bc  versus  either  relative  volume  or 
volumetric strain default:  LCBC = LCS); 
•  LCCA,  load  curve  number  for  sigma-ca  versus  either  relative  volume  or 
volumetric strain (default: LCCA = LCS);  
•  LCSR, optional load curve number for strain rate effects. 
The  behavior  before  compaction  is  orthotropic  where  the  components  of  the 
stress tensor are uncoupled, i.e., an 𝑎 component of strain will generate resistance in the 
local  𝑎  direction  with  no  coupling  to  the  local  𝑏  and  𝑐  directions.    The  elastic  moduli
(22.26.1) 
(22.26.2)
(22.26.3)
LS-DYNA Theory Manual 
Material Models 
vary  linearly  with  the  relative  volume  from  their  initial  values  to  the  fully  compacted 
values: 
𝐸𝑎𝑎 = 𝐸𝑎𝑎u + 𝛽(𝐸 − 𝐸𝑎𝑎u),
𝐸𝑏𝑏 = 𝐸𝑏𝑏u + 𝛽(𝐸 − 𝐸𝑏𝑏u), 
𝐸𝑐𝑐 = 𝐸𝑐𝑐u + 𝛽(𝐸 − 𝐸𝑐𝑐u), 
𝐺𝑎𝑏 = 𝐺𝑎𝑏u + 𝛽(𝐺 − 𝐺𝑎𝑏u), 
𝐺𝑏𝑐 = 𝐺𝑏𝑐u + 𝛽(𝐺 − 𝐺𝑏𝑐u), 
𝐺𝑐𝑎 = 𝐺𝑐𝑎u + 𝛽(𝐺 − 𝐺𝑐𝑎u),
𝛽 = max [min (
1 − 𝑉min
1 − 𝑉𝑓
, 1) ,0],
where 
and 𝐺 is the elastic shear modulus for the fully compacted honeycomb material 
𝐺 =
2(1 + 𝜈)
.
The  relative  volume  V  is  defined  as  the  ratio  of  the  current  volume  over  the 
initial volume; typically, 𝑉 = 1 at the beginning of a calculation.  The relative volume, 
𝑉min, is the minimum value reached during the calculation. 
The  load  curves  define  the  magnitude  of  the  average  stress  as  the  material 
changes density (relative volume).  Each curve related to this model must have the same 
Curve extends into negative volumetric 
strain quadrant since LS-DYNA will 
extrapolate using the two end points. It 
is important that the extropolation does 
not extend into the negative stress 
region.
ij
unloading and
reloading path
strain: -ε
ij
Unloading is based on the interpolated Young’s 
moduli which must provide an unloading 
tangent that exceeds the loading tangent.
Figure 22.26.1.  Stress quantity versus volumetric strain.  Note that the “yield 
stress” at a volumetric strain of zero is nonzero.  In the load curve definition, 
the “time” value is the volumetric strain and the “function” value is the yield 
stress.
Material Models 
LS-DYNA Theory Manual 
number  of  points  and  the  same  abscissa  values.    There  are  two  ways  to  define  these 
curves: as a function of relative volume V, or as a function of volumetric strain defined 
as: 
𝜀𝑉 = 1 − 𝑉.
(22.26.4)
In the former, the first value in the curve should correspond to a value of relative 
volume slightly less than the fully compacted value.  In the latter, the first value in the 
curve should be less than or equal to zero corresponding to tension and should increase 
to  full  compaction.    When  defining  the  curves,  care  should  be  taken  that  the 
extrapolated values do not lead to negative yield stresses. 
At  the  beginning  of the  stress  update  we  transform  each  element’s  stresses  and 
strain rates into the local element coordinate system.  For the uncompacted material, the 
trial stress components are updated using the elastic interpolated moduli according to: 
𝑛+1trial
𝑛+1trial
𝑛+1trial
𝑛+1trial
𝑛+1trial
𝑛+1trial
𝜎𝑎𝑎
𝜎𝑏𝑏
𝜎𝑐𝑐
𝜎𝑎𝑏
𝜎𝑏𝑐
𝜎𝑐𝑎
= 𝜎𝑎𝑎
= 𝜎𝑏𝑏
= 𝜎𝑐𝑐
= 𝜎𝑎𝑏
= 𝜎𝑏𝑐
= 𝜎𝑐𝑎
𝑛 + 𝐸𝑎𝑎Δ𝜀𝑎𝑎,
𝑛 + 𝐸𝑏𝑏Δ𝜀𝑏𝑏, 
𝑛 + 𝐸𝑐𝑐Δ𝜀𝑐𝑐, 
𝑛 + 2𝐺𝑎𝑏Δ𝜀𝑎𝑏, 
𝑛 + 2𝐺𝑏𝑐Δ𝜀𝑏𝑐, 
𝑛 + 2𝐺𝑐𝑎Δ𝜀𝑐𝑎 = 1.
(22.26.5)
Then we independently check each component of the updated stresses to ensure 
that they do not exceed the permissible values determined from the load curves, e.g., if 
then 
𝑛+1trial
∣𝜎𝑖𝑗
∣ > 𝜆𝜎𝑖𝑗(𝑉min),
𝑛+1 = 𝜎𝑖𝑗(𝑉min)
𝜎𝑖𝑗
𝑛+1trial
𝜆𝜎𝑖𝑗
𝑛+1trial∣
∣𝜎𝑖𝑗
. 
(22.26.6)
(22.26.7)
The  parameter  𝜆  is  either  unity  or  a  value  taken  from  the  load  curve  number, 
LCSR,  that  defines  𝜆  as  a  function  of  strain  rate.    Strain  rate  is  defined  here  as  the 
Euclidean norm of the deviatoric strain rate tensor. 
For  fully  compacted  material  we  assume  that  the  material  behavior  is  elastic-
perfectly plastic and updated the stress components according to 
trial = 𝑠𝑖𝑗
𝑠𝑖𝑗
𝑛 + 2𝐺Δ𝜀𝑖𝑗
dev𝑛+1
2⁄
,
(22.26.8)
where the deviatoric strain increment is defined as
LS-DYNA Theory Manual 
Material Models 
Δ𝜀𝑖𝑗
dev = Δ𝜀𝑖𝑗 −
Δ𝜀𝑘𝑘𝛿𝑖𝑗.
(22.26.9)
We  next  check  to  see  if  the  yield  stress  for  the  fully  compacted  material  is 
exceeded by comparing  
trial = (
𝑠eff
2⁄
trial)
trial𝑠𝑖𝑗
𝑠𝑖𝑗
.
(22.26.10)
the  effective  trial  stress,  to  the  yield  stress  𝜎y.    If  the  effective  trial  stress  exceeds  the 
yield stress, we simply scale back the stress components to the yield surface: 
𝑛+1 =
𝑠𝑖𝑗
𝜎y
trial
𝑠eff
trial.
𝑠𝑖𝑗
We can now update the pressure using the elastic bulk modulus, 𝐾: 
2⁄
𝑛+1
𝑝𝑛+1 = 𝑝𝑛 − 𝐾Δ𝜀𝑘𝑘
,
3(1 − 2𝜈)
𝐾 =
,
and obtain the final value for the Cauchy stress 
𝑛+1 = 𝑠𝑖𝑗
𝜎𝑖𝑗
𝑛+1 − 𝑝𝑛+1𝛿𝑖𝑗.
(22.26.11)
(22.26.12)
(22.26.13)
After completing the stress update, we transform the stresses back to the global 
configuration.
Material Models 
LS-DYNA Theory Manual 
22.27  Material Model 27:  Incompressible Mooney-Rivlin 
Rubber 
The  Mooney-Rivlin  material  model  is  based  on  a  strain  energy  function,  𝑊,  as 
follows  
𝑊 = A(𝐼1 − 3) + B(𝐼2 − 3) + C(
2 − 1) + D(𝐼3 − 1)2.
𝐼3
(22.27.1)
A and B are user defined constants, whereas C and D are related to A and B as 
follows 
C =
D =
A + B,
A(5𝜐 − 2) + B(11𝜐 − 5)
2(1 − 2𝜐)
.
(22.27.2)
The  derivation  of  the  constants  C  and  D  is  straightforward  [Feng,  1993]  and  is 
included  here  since  we  were  unable  to  locate  it  in  the  literature.    The  principal 
components of Cauchy stress, 𝜎𝑖, are given by [Ogden, 1984] 
For uniform dilation 
𝐽𝜎𝑖 = 𝜆𝑖
∂𝑊
∂𝜆𝑖
.
𝜆1 = 𝜆2 = 𝜆3 = 𝜆,
thus the pressure, 𝑝, is obtained (please note the sign convention), 
𝑝 = 𝜎1 = 𝜎2 = 𝜎3 =
𝜆3 (𝜆2 𝜕𝑊
𝜕𝐼1
+ 2𝜆4 𝜕𝑊
𝜕𝐼2
+ 𝜆6 𝜕𝑊
𝜕𝐼3
).
The relative volume, 𝑉, can be defined in terms of the stretches as: 
𝑉 = 𝜆3 =
new volume
old volume
.
(22.27.3)
(22.27.4)
(22.27.5)
(22.27.6)
For  small  volumetric  deformations  the  bulk  modulus,  𝐾,  can  be  defined  as  the 
ratio of the pressure over the volumetric strain as the relative volume approaches unity: 
𝑉 − 1
𝐾 = lim
𝑉→1
(22.27.7)
).
(
The partial derivatives of 𝑊 lead to:
LS-DYNA Theory Manual 
Material Models 
∂𝑊
∂𝐼1
𝜕𝑊
𝜕𝐼2
𝜕𝑊
𝜕𝐼3
= A, 
= B, 
= −2C𝐼3
−3 + 2D(𝐼3 − 1) = −2C𝜆−18 + 2D(𝜆6 − 1), 
(22.27.8)
𝑝 =
=
𝜆3 {A𝜆2 + 2𝜆4B + 𝜆6[−2C𝜆−18 + 2D(𝜆6 − 1)]} 
𝜆3 {A𝜆2 + 2𝜆4B − 2C𝜆−12 + 2D(𝜆12 − 𝜆6)}. 
In  the  limit  as  the  stretch  ratio  approaches  unity,  the  pressure  must  approach 
zero: 
lim
𝜆→1
𝑝 = 0.
(22.27.9)
Therefore, A + 2B − 2C = 0 and 
C = 0.5A + B.
(22.27.10)
To solve for D we note that: 
) 
(
𝑉 − 1
𝜆3 {A𝜆2 + 2𝜆4B − 2C𝜆−12 + 2D(𝜆12 − 𝜆6)}
𝜆3 − 1
A𝜆2 + 2𝜆4B − 2C𝜆−12 + 2D(𝜆12 − 𝜆6)
𝜆6 − 𝜆3
2A𝜆 + 8𝜆3B + 24C𝜆−13 + 2D(12𝜆11 − 6𝜆5)
6𝜆5 − 3𝜆2
(2A + 8B + 24C + 12D) 
(14A + 32B + 12D).
𝐾 = lim
𝑉→1
= lim
λ→1
= 2lim
λ→1
= 2lim
λ→1
=
=
We therefore obtain: 
14A + 32B + 12D =
𝐾 =
(
2𝐺(1 + 𝜐)
3(1 − 2𝜐)
) =
2(A + B)(1 + 𝜐)
(1 − 2𝜐)
. 
Solving for D we obtain the desired equation: 
D =
A(5𝜐 − 2) + B(11𝜐 − 5)
2(1 − 2𝜐)
.
(22.27.11)
(22.27.12)
(22.27.13)
Material Models 
LS-DYNA Theory Manual 
The invariants 𝐼1 − 𝐼3 are related to the right Cauchy-Green tensor C as 
𝐼1 = 𝐶𝑖𝑖,
2 −
𝐼2 =
𝐶𝑖𝑖
𝐼3 = det(𝐶𝑖𝑗).
𝐶𝑖𝑗𝐶𝑖𝑗, 
(22.27.14)
The  second  Piola-Kirchhoff  stress  tensor,  S,  is  found  by  taking  the  partial 
derivative  of  the  strain  energy  function  with  respect  to  the  Green-Lagrange  strain 
tensor, E. 
𝑆𝑖𝑗 =
∂𝑊
∂𝐸𝑖𝑗
= 2
∂𝑊
∂𝐶𝑖𝑗
= 2 [A
∂𝐼1
∂𝐶𝑖𝑗
+ B
∂𝐼2
∂𝐶𝑖𝑗
+ (2D(𝐼3 − 1) −
2C
2 )
𝐼3
∂I3
∂𝐶𝑖𝑗
]. 
(22.27.15)
The derivatives of the invariants 𝐼1 − 𝐼3 are 
∂𝐼1
∂𝐶𝑖𝑗
∂𝐼2
∂𝐶𝑖𝑗
∂𝐼3
∂𝐶𝑖𝑗
= 𝛿𝑖𝑗,
= 𝐼1𝛿𝑖𝑗 − 𝐶𝑖𝑗, 
= 𝐼3𝐶𝑖𝑗
−1.
(22.27.16)
Inserting  Equation  (22.27.16)  into  Equation  (22.27.15)  yields  the  following 
expression for the second Piola-Kirchhoff stress: 
𝑆𝑖𝑗 = 2A𝛿𝑖𝑗 + 2B(𝐼1𝛿𝑖𝑗 − 𝐶𝑖𝑗) − 4C
2 𝐶𝑖𝑗
𝐼3
Equation  (22.27.17)  can  be  transformed  into  the  Cauchy  stress  by  using  the  push 
forward operation 
−1 + 4D(𝐼3 − 1)I3𝐶𝑖𝑗
(22.27.17)
−1. 
𝜎𝑖𝑗 =
𝐹𝑖𝑘𝑆𝑘𝑙𝐹𝑗𝑙.
(22.27.18)
where 𝐽 = det(𝐹𝑖𝑗). 
22.27.1  Stress Update for Shell Elements 
As  a  basis  for  discussing  the  algorithmic  tangent  stiffness  for  shell  elements  in 
Section  19.27.3,  the  corresponding  stress  update  as  it  is  done  in  LS-DYNA  is  shortly 
recapitulated  in  this  section.    When  dealing  with  shell  elements,  the  stress  (as  well  as 
constitutive  matrix)  is  typically  evaluated  in  corotational  coordinates  after  which  it  is 
transformed back to the standard basis according to 
22-94 (Material Models) 
𝜎𝑖𝑗 = 𝑅𝑖𝑘𝑅𝑗𝑙𝜎̂𝑘𝑙.
LS-DYNA Theory Manual 
Material Models 
Here 𝑅𝑖𝑗 is the rotation matrix containing the corotational basis vectors.  The so-
called  corotated  stress 𝜎̂𝑖𝑗  is  evaluated  using  Equation 19.27.21  with  the  exception  that 
the deformation gradient is expressed in the corotational coordinates, i.e., 
𝜎̂𝑖𝑗 =
𝐹̂𝑖𝑘𝑆𝑘𝑙𝐹̂𝑗𝑙,
(22.27.20)
where 𝑆𝑖𝑗 is evaluated using Equation (22.27.17). The corotated deformation gradient is 
incrementally  updated  with  the  aid  of  a  time  increment  Δ𝑡,  the  corotated  velocity 
gradient 𝐿̂ 𝑖𝑗, and the angular velocity 𝛺̂𝑖𝑗 with which the embedded coordinate system 
is rotating. 
𝐹̂𝑖𝑗 = (𝛿𝑖𝑘 + Δ𝑡𝐿̂ 𝑖𝑘 − Δ𝑡𝛺̂𝑖𝑘)𝐹̂𝑘𝑗.
(22.27.21)
The  primary  reason  for  taking  a  corotational  approach  is  to  facilitate  the 
maintenance of a vanishing normal stress through the thickness of the shell, something 
that  is  achieved  by  adjusting  the  corresponding  component  of  the  corotated  velocity 
gradient 𝐿̂ 33 accordingly.  The problem can be stated as to determine 𝐿̂ 33 such that when 
updating  the  deformation  gradient  through  Equation  (22.27.21)  and  subsequently  the 
stress through Equation (22.27.20), 𝜎̂33 = 0.  To this end, it is assumed that 
𝐿̂ 33 = 𝛼(𝐿̂ 11 + 𝐿̂ 22),
(22.27.22)
for some parameter α that is determined in the following three step procedure.  In the 
(0) 
first two steps, 𝛼 = 0 and 𝛼 = −1, respectively, resulting in two trial normal stresses 𝜎̂33
(−1).  Then  it  is  assumed  that  the  actual  normal  stress  depends  linearly  on  𝛼, 
and  𝜎̂33
meaning that the latter can be determined from 
0 = 𝜎33
(𝛼) = 𝜎33
(0) + 𝛼(𝜎33
(0) − 𝜎33
(−1)).
In LS-DYNA, α is given by 
(0)
𝜎̂33
(−1) − 𝜎̂33
𝜎̂33
(0)
∣𝜎̂33
(−1) − 𝜎̂33
(0)∣ ≥ 10−4
− 1
otherwise
𝛼 =
⎧
{
{
{
⎨
{
{
{
⎩
(22.27.23)
, 
(22.27.24)
and  the  stresses  are  determined  from  this  value  of  α.  Finally,  to  make  sure  that  the 
normal stress through the thickness vanishes, it is set to 0 (zero) before exiting the stress 
update routine. 
22.27.2  Derivation of the Continuum Tangent Stiffness 
This  section  will  describe  the  derivation  of  the  continuum  tangent  stiffness  for 
the  Mooney-Rivlin  material.    For  solid  elements,  the  continuum  tangent  stiffness  is
Material Models 
LS-DYNA Theory Manual 
chosen  in  favor  of  an  algorithmic  (consistent)  tangential  modulus  as  the  constitutive 
equation at hand is smooth and a consistent tangent modulus is not required for good 
convergence  properties.    For  shell  elements  however,  this  stiffness  must  ideally  be 
modified  in  order  to  account  for  the  zero  normal  stress  condition.    This  modification, 
and its consequences, are discussed in the next section. 
The continuum tangent modulus in the reference configuration is per definition, 
PK =
𝐸𝑖𝑗𝑘𝑙
∂𝑆𝑖𝑗
∂𝐸𝑘𝑙
= 2
∂𝑆𝑖𝑗
∂𝐶𝑘𝑙
.
Splitting up the differentiation of Equation (22.27.17) we get 
∂(𝐼1𝛿𝑖𝑗 − 𝐶𝑖𝑗)
∂𝐶𝑘𝑙
= 𝛿𝑘𝑙𝛿𝑖𝑗 −
(𝛿𝑖𝑘𝛿𝑗𝑙 + 𝛿𝑖𝑙𝛿𝑗𝑘)
−1)
𝜕 ( 1
2 𝐶𝑖𝑗
𝐼3
𝜕𝐶𝑘𝑙
= −
2 𝐶𝑘𝑙
𝐼3
−1𝐶𝑖𝑗
−1 −
2 (𝐶𝑘𝑗
2𝐼3
−1𝐶𝑖𝑙
−1 + 𝐶𝑙𝑗
−1𝐶𝑖𝑘
−1)
𝜕(𝐼3(𝐼3 − 1)𝐶𝑖𝑗
𝜕𝐶𝑘𝑙
−1)
= 𝐼3(2𝐼3 − 1)𝐶𝑘𝑙
−1𝐶𝑖𝑗
−1 −
𝐼3(𝐼3 − 1)(𝐶𝑘𝑗
−1𝐶𝑖𝑙
−1 + 𝐶𝑙𝑗
−1𝐶𝑖𝑘
−1). 
(22.27.25)
(22.27.26)
(22.27.27)
(22.27.28)
Since LS-DYNA needs the tangential modulus for the Cauchy stress, it is a good 
idea to transform the terms in Equation (22.27.27) before summing them up.  The push 
forward operation for the fourth-order tensor 𝐸𝑖𝑗𝑘𝑙
pk  is 
TC =
𝐸𝑖𝑗𝑘𝑙
PK .
𝐹𝑖𝑎𝐹𝑗𝑏𝐹𝑘𝑐𝐹𝑙𝑑𝐸𝑎𝑏𝑐𝑑
(22.27.29)
Since the right Cauchy-Green tensor is 𝐂 = 𝐅T𝐅 and the left Cauchy-Green tensor 
is  𝐛 = 𝐅T𝐅,  and  the  determinant  and  trace  of  the  both  stretches  are  equal,  the 
transformation is in practice carried out by interchanging 
−1 → 𝛿𝑖𝑗,
𝐶𝑖𝑗
𝛿𝑖𝑗 → 𝑏𝑖𝑗.
(22.27.30)
(22.27.31)
The end result is then
LS-DYNA Theory Manual 
Material Models 
𝐽𝐸𝑖𝑗𝑘𝑙
TC = 4B [𝑏𝑘𝑙𝑏𝑖𝑗 −
(𝑏𝑖𝑘𝑏𝑗𝑙 + 𝑏𝑖𝑙𝑏𝑗𝑘)] +
4C
2 [4𝛿𝑖𝑗𝛿𝑘𝑙 + (𝛿𝑘𝑗𝛿𝑖𝑙 + 𝛿𝑙𝑗𝛿𝑖𝑚)] + 
I3
(22.27.32)
8D𝐼3 [(2𝐼3 − 1)𝛿𝑖𝑗𝛿𝑘𝑙 −
(𝐼3 − 1)(𝛿𝑘𝑗𝛿𝑖𝑙 + 𝛿𝑙𝑗𝛿𝑖𝑘)]. 
22.27.3  The Algorithmic Tangent Stiffness for Shell Elements 
The  corotated  tangent  stiffness  matrix  is  given  by  Equation  (22.27.32)  with  the 
exception  that  the  left  Cauchy-Green  tensor  and  deformation  gradient  are  given  in 
corotational coordinates, i.e., 
𝐽𝐸̂
TC = 4B [𝑏̂
𝑖𝑗𝑘𝑙
𝑘𝑙𝑏̂
𝑖𝑗 −
(𝑏̂
𝑖𝑘𝑏̂
𝑗𝑙 + 𝑏̂
𝑖𝑙𝑏̂
𝑗𝑘)] +
+  8D𝐼3 [(2𝐼3 − 1)𝛿𝑖𝑗𝛿𝑘𝑙 −
4C
2 [4𝛿𝑖𝑗𝛿𝑘𝑙 + (𝛿𝑘𝑗𝛿𝑖𝑙 + 𝛿𝑙𝑗𝛿𝑖𝑚)]
𝐼3
(𝐼3 − 1)(𝛿𝑘𝑗𝛿𝑖𝑙 + 𝛿𝑙𝑗𝛿𝑖𝑘)]. 
(22.27.33)
Using this exact expression for the tangent stiffness matrix in the context of shell 
elements is not adequate since it does not take into account that the normal stress is zero 
and it must be modified appropriately.  To this end, we assume that the tangent moduli 
in  Equation  (22.27.33)  relates  the  corotated  rate-of-deformation  tensor  𝐷̂ 𝑖𝑗  to  the 
•, 
corotated rate of stress 𝜎̂𝑖𝑗
• = 𝐸̂
𝜎̂𝑖𝑗
TC𝐷̂ 𝑘𝑙.
𝑖𝑗𝑘𝑙
(22.27.34)
Even  though  this  is  not  completely  true,  we  believe  that  attempting  a  more 
thorough treatment would hardly be worth the effort.  The objective can now be stated 
as to find a modified tangent stiffness matrix 𝐸̂
TCalg such that 
ijkl
•alg = 𝐸̂
𝜎̂𝑖𝑗
TCalg𝐷̂ 𝑘𝑙,
𝑖𝑗𝑘𝑙
(22.27.35)
alg is the stress as it is evaluated in LS-DYNA.  The stress update, described in 
where 𝜎̂𝑖𝑗
Section  19.27.1,  is  performed  in  a  rather  ad hoc  way  which  probably  makes  the  stated 
objective  unachievable.    Still  we  attempt  to  extract  relevant  information  from  it  that 
enables us to come somewhat close.  
An  example  of  a  modification  of this  tangent  moduli  is  due  to  Hughes  and  Liu 
[1981] and given by 
𝐸̂
TCalg = 𝐸̂
𝑖𝑗𝑘𝑙
TC −
𝑖𝑗𝑘𝑙
TC
33𝑘𝑙
TC 𝐸̂
𝐸̂𝑖𝑗33
𝐸̂
TC
3333
.
(22.27.36)
Material Models 
LS-DYNA Theory Manual 
This matrix is derived by eliminating the thickness strain 𝐷̂ 33 from the equation 
• = 0  in  Equation  (22.27.35)  as  an  unknown.    This  modification  is  unfortunately  not 
𝜎̂33
consistent  with  how  the  stresses  are  updated  in  LS-DYNA.  When  consulting  Section 
19.27.1, it is suggested that 𝐷̂ 33 instead can be eliminated from 
𝐷̂ 33 = 𝛼(𝐷̂ 11 + 𝐷̂ 22),
(22.27.37)
using  the  α  determined  from  the  stress  update.    Unfortunately,  by  the  time  when  the 
tangent  stiffness  matrix  is  calculated,  the  exact  value  of  α  is  not  known.    From 
experimental  observations  however,  we  have  found  that  α  is  seldom  far  from  being 
equal  to  −1.    The  fact  that  α = −1  represents  incompressibility  strengthen  this 
TC except 
hypothesis.  This leads to a modified tangent stiffness 𝐸̂
𝑖𝑗𝑘𝑙
for the following modifications, 
TCalg that is equal to 𝐸̂
𝑖𝑗𝑘𝑙
𝐸̂
𝐸̂
TCalg = 𝐸̂𝑖𝑖𝑗𝑗
𝑖𝑖𝑗𝑗
TCalg = 𝐸̂
33𝑖𝑗
TC − 𝐸̂33𝑗𝑗
TC − 𝐸̂𝑖𝑖33
TCalg = 0, 𝑖 ≠ 𝑗.
𝑖𝑗33
TC ,
TC + 𝐸̂3333
(22.27.38)
To preclude the obvious singularity, a small positive value is assigned to 𝐸̂
TCalg, 
3333
𝐸̂
TCalg = 10−4(∣𝐸̂
3333
TCalg∣ + ∣𝐸̂
1111
TCalg∣).
2222
(22.27.39)
As with the Hughes-Liu modification, this modification preserves symmetry and 
positive  definiteness  of  the  tangent  moduli,  which  together  with  the  stress  update 
“consistency” makes it intuitively attractive.
LS-DYNA Theory Manual 
Material Models 
22.28  Material Model 28:  Resultant Plasticity 
This plasticity model, based on resultants as illustrated in Figure 22.28.1, is very 
cost  effective  but  not  as  accurate  as  through-thickness  integration.    This  model  is 
available  only  with  the  C0  triangular,  Belytschko-Tsay  shell,  and  the  Belytschko  beam 
element  since  these  elements,  unlike  the  Hughes-Liu  elements,  lend  themselves  very 
cleanly to a resultant formulation.  
(a)
Membrane
(b)
Bending
Figure 22.28.1.  Full section yield using resultant plasticity. 
In applying this model to shell elements the resultants are updated incrementally 
using the midplane strains 𝜀m and curvatures 𝜅: 
Δ𝑛 = Δ𝑡𝐶𝜀m
Δ𝑚 = Δ𝑡
ℎ3
12
𝐶𝜅,
(22.28.1) 
(22.28.2) 
where the plane stress constitutive matrix is given in terms of Young’s Modulus 𝐸 and 
Poisson’s ratio 𝜈 as: 
𝑚̅̅̅̅̅ = 𝑚𝑥𝑥
2 − 𝑚𝑥𝑥𝑚𝑦𝑦 + 𝑚𝑦𝑦
2 .
2 + 3𝑚𝑥𝑦
Defining 
𝑛̅ = 𝑛𝑥𝑥
2 − 𝑛𝑥𝑥𝑛𝑦𝑦 + 𝑛𝑦𝑦
2 ,
2 + 3𝑛𝑥𝑦
𝑚̅̅̅̅̅ = 𝑚𝑥𝑥
2 − 𝑚𝑥𝑥𝑚𝑦𝑦 + 𝑚𝑦𝑦
2 ,
2 + 3𝑚𝑥𝑦
𝑚̅̅̅̅̅𝑛̅ = 𝑚𝑥𝑥𝑛𝑥𝑥 −
𝑚𝑥𝑥𝑛𝑦𝑦 −
𝑛𝑥𝑥𝑚𝑦𝑦 + 𝑚𝑦𝑛𝑦 + 3𝑚𝑥𝑦𝑛𝑥𝑦,
the Ilyushin yield function becomes 
𝑓 (𝑚, 𝑛) = 𝑛̅ +
4|𝑚̅̅̅̅̅𝑛̅|
ℎ√3
+
16𝑚̅̅̅̅̅
ℎ2 ≤ 𝑛y
2 = ℎ2𝜎y
2.
(22.28.3)
(22.28.4) 
(22.28.5) 
(22.28.6) 
(22.28.7)
Material Models 
LS-DYNA Theory Manual 
In our implementation we update the resultants elastically and check to see if the yield 
condition is violated: 
If so, the resultants are scaled by the factor 𝛼: 
2.
𝑓 (𝑚, 𝑛) > 𝑛y
𝛼 = √
𝑛y
.
𝑓 (𝑚, 𝑛)
We update the yield stress incrementally: 
(22.28.8)
(22.28.9)
𝑛 + 𝐸PΔ𝜀plastic
where  𝐸P  is  the  plastic  hardening  modulus  which  in  incremental  plastic  strain  is 
approximated by 
𝑛+1 = 𝜎y
𝜎y
(22.28.10)
eff
,
eff
Δ𝜀plastic
=
√𝑓 (𝑚, 𝑛) − 𝑛y
ℎ(3𝐺 + 𝐸𝑝)
.
(22.28.11)
Kennedy,  et.    al.,  report  that  this  model  predicts  results  that  may  be  too  stiff; 
users of this model should proceed cautiously. 
In applying this material model to the Belytschko beam, the flow rule changes to 
𝑓 (𝑚, 𝑛) = 𝑓 ̂
2 +
2𝐴
4𝑚̂𝑦
3𝐼𝑦𝑦
+
2𝐴
4𝑚̂𝑧
3𝐼𝑧𝑧
≤ 𝑛y
2,
2 = 𝐴2𝜎y
(22.28.12)
have been updated elastically according to Equations (4.16)-(4.18).  The yield condition 
is  checked  with  Equation  (22.28.8),  and  if  it  is  violated,  the  resultants  are  scaled  as 
described above. 
This  model  is  frequently  applied  to  beams  with  non-rectangular  cross  sections.  
The  accuracy  of  the  results  obtained  should  be  viewed  with  some  healthy  suspicion.  
No work hardening is available with this model.
LS-DYNA Theory Manual 
Material Models 
22.29  Material Model 29:  FORCE LIMITED Resultant 
Formulation 
This  material  model  is  available  for  the  Belytschko  beam  element  only.    Plastic 
hinges form at the ends of the beam when the moment reaches the plastic moment.  The 
moment-versus-rotation relationship is specified by the user in the form of a load curve 
and scale factor.  The point pairs of the load curve are (plastic rotation in radians, plastic 
moment).  Both quantities should be positive for all points, with the first point pair being 
(zero,  initial  plastic  moment).    Within  this  constraint  any  form  of  characteristic  may  be 
used  including  flat  or  falling  curves.    Different  load  curves  and  scale  factors  may  be 
specified at each node and about each of the local s and t axes. 
Axial collapse occurs when the compressive axial load reaches the collapse load.  
The collapse load-versus-collapse deflection is specified in the form of a load curve.  The 
points of the load curve are (true strain, collapse force).  Both quantities should be entered 
as positive for all points, and will be interpreted as compressive i.e., collapse does not 
occur in tension.  The first point should be the pair (zero, initial collapse load). 
The collapse load may vary with end moment and with deflection.  In this case, 
several  load-deflection  curves  are  defined,  each  corresponding  to  a  different  end 
moment.    Each  load  curve  should  have  the  same  number  of  point  pairs  and  the  same 
deflection values.  The end moment is defined as the average of the absolute moments 
at  each  end  of  the  beam,  and  is  always  positive.    It  is  not  possible  to  make the  plastic 
moment vary with axial load. 
A  co-rotational  technique  and  moment-curvature  relations  are  used  to  compute 
the internal forces.  The co-rotational technique is treated in Section 4 in and will not be 
treated  here  as  we  will  focus  solely  on  the  internal  force  update  and  computing  the 
tangent stiffness.  For this we use the notation
Material Models 
LS-DYNA Theory Manual 
M8
M7
M6
M5
M4
M3
M2
M1M1
Strain (or change in length, see AOPT)
Figure  22.29.1.    The  force  magnitude  is  limited  by  the  applied  end  moment.
For an intermediate value of the end moment, LS-DYNA interpolates between 
the curves to determine the allowable force. 
𝐸 = Young′smodulus 
𝐺 = Shear modulus 
𝐴 = Cross sectional area 
𝐴s = Effective area in shear 
𝑙𝑛 = Reference length of beam 
𝑙𝑛+1 = Current length of beam 
𝐼𝑦𝑦 = Second moment of inertia about 𝑦 
𝐼𝑧𝑧 = Second moment of inertia about 𝑧 
𝐽 = Polar moment of inertia 
𝑒𝑖 = 𝑖th local base vector in the current configuration 
𝑦𝐼 = nodal vector in y direction at node I in the current configuration 
𝑧𝐼 = nodal vector in z direction at node I in the current configuration 
(22.29.1)
LS-DYNA Theory Manual 
Material Models 
We  emphasize  that  the  local 𝑦  and  𝑧  base  vectors  in  the  reference  configuration 
always coincide with the corresponding nodal vectors.  The nodal vectors in the current 
configuration are updated using the Hughes-Winget formula while the base vectors are 
computed from the current geometry of the element and the current nodal vectors. 
22.29.1  Internal Forces 
Elastic Update 
In  the  local  system  for  a  beam  connected  by  nodes  I  and  J,  the  axial  force  is 
updated as 
where 
el = 𝐟a
𝐟a
n + Ka
el𝛅,
𝐾a
𝐸𝐴
el =
𝑙𝑛 ,
𝛿 = 𝑙𝑛+1 − 𝑙𝑛.
The torsional moment is updated as 
𝑚t
el = 𝑚t
n + 𝐾t
el𝜃t,
where 
el =
𝐾t
𝜃t =
𝐺𝐽
𝑙𝑛 ,
T(𝐲I × 𝐲J + 𝐳I × 𝐳J).
𝐞1
The bending moments are updated as 
n + 𝐀𝑦
el = 𝐦𝑦
𝐦𝑦
el𝛉𝑦
𝐦𝑧
el = 𝐦𝑧
n + 𝐀𝑧
el𝛉𝑧,
where 
el =
𝐀∗
1 + 𝜑∗
𝐸𝐼∗∗
𝑙n [
4 + 𝜑∗
2 − 𝜑∗
2 − 𝜑∗
4 + 𝜑∗
]
𝜑∗ =
12𝐸𝐼∗∗
𝐺𝐴slnln
T = −𝐞3
𝛉y
T(𝐲I × 𝐳I 𝐲J × 𝐳J)
T = 𝐞2
𝛉z
T(𝐲I × 𝐳I 𝐲J × 𝐳J).
(22.29.2)
(22.29.3) 
(22.29.4)
(22.29.5) 
(22.29.6) 
(22.29.7) 
(22.29.8) 
(22.29.9) 
(22.29.10)
(22.29.11)
In the following we refer to 𝐀∗
el as the (elastic) moment-rotation matrix.
Material Models 
Plastic Correction 
LS-DYNA Theory Manual 
After the elastic update the state of force is checked for yielding as follows.  As a 
preliminary  note  we  emphasize  that  whenever  yielding  does  not  occur  the  elastic 
stiffnesses and forces are taken as the new stiffnesses and forces. 
Y(𝜃𝑖𝐼
The  yield  moments  in  direction  𝑖  at  node  𝐼  as  functions  of  plastic  rotations  are 
P).  This  function  is  given  by  the  user  but  also  depends  on  whether  a 
denoted  𝑚𝑖𝐼
plastic hinge has been created.  The theory for plastic hinges is given in the LS-DYNA 
Keyword User’s Manual [Hallquist 2003] and is not treated here.  Whenever the elastic 
moment exceeds the plastic moment, the plastic rotations are updated as 
P(𝑛+1) = 𝜃𝑖𝐼
𝜃𝑖𝐼
P(𝑛) +
∣𝑚𝑖𝐼
el∣ − 𝑚𝑖𝐼
max (0.001, 𝐴𝑖(𝐼𝐼)
el +
, 
∂𝑚𝑖𝐼
P )
∂𝜃𝑖𝐼
and the moment is reduced to the yield moment 
𝑚𝑖𝐼
𝑛+1 = 𝑚𝑖𝐼
Y(𝜃𝑖𝐼
P(𝑛+1))sgn(𝑚𝑖𝐼
el).
(22.29.12)
(22.29.13)
The  corresponding  diagonal  component  in  the  moment-rotation  matrix  is 
reduced as 
𝑛+1 = 𝐴𝑖(𝐼𝐼)
𝐴𝑖(II)
el
1 − 𝛼
⎜⎜⎜⎜⎜⎜⎜⎜⎛
⎝
el
𝐴𝑖(𝐼𝐼)
max (0.001, 𝐴𝑖(𝐼𝐼)
el +
, 
⎟⎟⎟⎟⎟⎟⎟⎟⎞
⎠
∂𝑚𝑖𝐼
P )
∂𝜃𝑖𝐼
(22.29.14)
where  α ≤ 1  is  a  parameter  chosen  such  that  the  moment-rotation  matrix  remains 
positive definite. 
The yield moment in torsion is given by 𝑚t
P) and is provided by the user.  If 
the elastic torsional moment exceeds this value, the plastic torsional rotation is updated 
as 
Y(𝜃t
P(𝑛+1) = 𝜃t
𝜃t
P(𝑛) +
∣𝑚t
el∣ − 𝑚t
max (0.001, 𝐾t
el +
, 
∂𝑚t
P )
∂𝜃t
and the moment is reduced to the yield moment 
𝑚t
𝑛+1 = 𝑚t
Y(𝜃t
P(𝑛+1))sgn(𝑚t
el).
(22.29.15)
(22.29.16)
The torsional stiffness is modified as
LS-DYNA Theory Manual 
Material Models 
𝐾t
el
n+1 = 𝐾t
1 − α
⎜⎜⎜⎜⎜⎜⎜⎜⎛
⎝
el
𝐾t
⎟⎟⎟⎟⎟⎟⎟⎟⎞
∂𝑚t
∂𝜃t
P ⎠
el +
𝐾t
, 
(22.29.17)
where again α ≤ 1 is chosen so that the stiffness is positive. 
Axial collapse is modeled by limiting the axial force by 𝑓a
Y(𝜀, 𝑚), i.e., a function of 
the  axial  strains  and  the  magnitude  of  bending  moments.    If  the  axial  elastic  force 
exceeds this value it is reduced to yield 
𝑛+1 = 𝑓a
𝑓a
and the axial stiffness is given by 
Y(𝜀𝑛+1, 𝑚𝑛+1)sgn(𝑓a
el),
𝐾a
el,
𝑛+1 = max (0.05𝐾a
∂𝑓a
∂𝜀
).
(22.29.18)
(22.29.19)
We  neglect  the  influence  of  change  in  bending  moments  when  computing  this 
parameter. 
Damping 
Damping is introduced by adding a viscous term to the internal force on the form 
𝐟v = 𝐃
𝑑𝑡
⎤
⎡
𝜃t
⎥
⎢
, 
⎥
⎢
𝜃𝑦
⎥
⎢
𝜃𝑧⎦
⎣
𝐃 = 𝛾
el
⎡𝐾a
⎢
⎢
⎢
⎢
⎣
el
𝐾t
el
𝐴𝑦
⎤
⎥
⎥
, 
⎥
⎥
el⎦
𝐴𝑧
(22.29.20)
(22.29.21)
where γ is a damping parameter. 
Transformation 
The  internal  force  vector  in  the  global  system  is  obtained  through  the 
transformation 
where 
𝑛+1 = 𝐒𝐟l
𝐟g
𝑛+1,
(22.29.22)
Material Models 
LS-DYNA Theory Manual 
−𝑒3/𝑙𝑛+1 −𝑒3/𝑙𝑛+1
𝐒 =
−𝑒1
⎡
⎢
⎢
𝑒1
⎢
⎣
−𝑒1
𝑒1
𝑒2
𝑒3/𝑙𝑛+1
𝑒2/𝑙𝑛+1
𝑒3
𝑒3/𝑙𝑛+1 −𝑒2/𝑙𝑛+1 −𝑒2/𝑙𝑛+1
𝑒2/𝑙𝑛+1
𝑒2
𝑒3
𝑛+1 =
𝐟l
𝑛+1
𝑛+1
fa
⎡
⎢
𝑚t
⎢
⎢
𝑚y
⎢
𝑚z
⎣
⎤
⎥
⎥
⎥
⎥
𝑛+1⎦
𝑛+1
. 
⎤
⎥
, 
⎥
⎥
⎦
(22.29.23)
(22.29.24)
22.29.2  Tangent Stiffness 
Derivation 
The tangent stiffness is derived from taking the variation of the internal force 
δ𝐟g
𝑛+1 = δ𝐒𝐟l
𝑛+1 + 𝐒δ𝐟l
𝑛+1,
which can be written 
where  
𝑛+1 = 𝐊geoδ𝐮 + 𝐊matδ𝐮,
δ𝐟g
δ𝐮 = [δx𝐼
δω𝐼
δx𝐽
δω𝐽
T]
.
(22.29.25)
(22.29.26)
(22.29.27)
There  are  two  contributions  to  the  tangent  stiffness,  one  geometrical  and  one 
material contribution.  The geometrical contribution is given (approximately) by 
𝐊geo = 𝐑(𝐟l
𝑛+1 ⊗ 𝐈)𝐖 −
l𝑛+1l𝑛+1 𝐓𝐟l
𝑛+1𝐋,
where 
𝐑 =
𝑅1
⎡
⎢
⎢
−𝑅1
⎢
⎣
𝑅1
−𝑅1
𝑅3/𝑙𝑛+1
−𝑅2
𝑅3/𝑙𝑛+1 −𝑅2/𝑙𝑛+1 −𝑅2/𝑙𝑛+1
−𝑅3
𝑅2/𝑙𝑛+1
𝑅2/𝑙𝑛+1
−𝑅3
−𝑅2
−𝑅3/𝑙𝑛+1 −𝑅3/𝑙𝑛+1
𝐖 = [−𝑅1/𝑙𝑛+1
𝐞1𝐞1
T/2 𝑅1/𝑙𝑛+1
𝐞1𝐞1
T/2],
𝐓 =
⎡
⎢
⎢
⎣
𝑒2
0 −𝑒3 −𝑒3
𝑒2
⎤
⎥
, 
⎥
𝑒3
𝑒3 −𝑒2 −𝑒2
0 ⎦
𝐋 = [−𝐞1
𝐞1
0],
⎤
⎥
, 
⎥
⎥
⎦
(22.29.28)
(22.29.29)
(22.29.30)
(22.29.31)
(22.29.32)
and 𝐈 is the 3 by 3 identity matrix.  We use ⊗ as the outer matrix product and define
LS-DYNA Theory Manual 
Material Models 
Riv = 𝐞i × 𝐯.
The material contribution can be written as 
𝐊mat = 𝐒𝐊𝐒T,
where 
𝐊 =
𝑛+1
𝐾a
⎡
⎢
⎢
⎢
⎢
⎣
𝑛+1
𝐾t
𝑛+1
𝐴y
⎤
⎥
⎥
⎥
⎥
𝑛+1⎦
𝐴z
+
Δ𝑡
𝐃. 
(22.29.33)
(22.29.34)
(22.29.35)
Material Models 
LS-DYNA Theory Manual 
22.30  Material Model 30:  Closed-Form Update Shell 
Plasticity 
This  section  presents  the  mathematical  details  of  the  shape  memory  alloy 
material in LS-DYNA. The description closely follows the one of Auricchio and Taylor 
[1997] with appropriate modifications for this particular implementation. 
22.30.1  Mathematical Description of the Material Model 
The Kirchhoff stress 𝛕 in the shape memory alloy can be written 
where 𝐢 is the second order identity tensor and 
𝛕 = 𝑝𝐢 + 𝐭,
𝑝 = 𝐾(𝜃 − 3α𝜉S𝜀L),
𝐭 = 2𝐺(𝐞 − 𝜉S𝜀L𝐧).
(22.30.1)
(22.30.2) 
(22.30.3) 
Here  𝐾  and  𝐺  are  bulk  and  shear  modulii,  𝜃  and  e  are  volumetric  and  shear 
logarithmic strains and 𝛼 and 𝜀L are constant material parameters.  There is an option to 
define the bulk and shear modulii as functions of the martensite fraction according to 
𝐾 = 𝐾A + 𝜉S(𝐾S − 𝐾A),
𝐺 = 𝐺A + 𝜉S(𝐺S − 𝐺A),
(22.30.4)
in case the stiffness of the martensite differs from that of the austenite.  Furthermore, the 
unit vector 𝐧 is defined as 
and a loading function is introduced as 
𝐧 = 𝐞/(‖𝐞‖ + 10−12),
where 
𝐹 = 2𝐺‖𝐞‖ + 3𝛼𝐾𝜃 − 𝛽𝜉S,
𝛽 = (2𝐺 + 9𝛼2𝐾)𝜀L.
(22.30.5)
(22.30.6)
(22.30.7)
For the evolution of the martensite fraction 𝜉S in the material, the following rule 
is adopted 
AS > 0
𝐹 − 𝑅s
𝐹̇ > 0
𝜉S < 1
}⎫
}⎬
⎭
     ⇒      𝜉 ̇
S = −(1 − 𝜉S)
𝐹̇
𝐹 − 𝑅f
AS
(22.30.8)
LS-DYNA Theory Manual 
Material Models 
SA < 0
𝐹 − 𝑅s
𝐹̇ < 0
𝜉S > 0
}⎫
}⎬
⎭
     ⇒      𝜉 ̇
S = 𝜉S
𝐹̇
𝐹 − 𝑅f
SA
. 
(22.30.9)
AS,  𝑅s
stress is finally obtained as 
Here  𝑅s
AS,  𝑅f
SA  and  𝑅f
SA  are  constant  material  parameters.    The  Cauchy 
𝛔 =
,
(22.30.10)
where 𝐽 is the Jacobian of the deformation. 
22.30.2  Algorithmic Stress Update 
For the stress update we assume that the martensite fraction 𝜉S
𝑛 and the value of 
the  loading  function  F𝑛  is  known  from  time  𝑡𝑛  and  the  deformation  gradient  at  time 
𝑡𝑛+1,  F,  is  known.    We  form  the  left  Cauchy-Green  tensor  as  𝐁 = 𝐅𝐅Twhich  is 
diagonalized  to  obtain  the  principal  values  and  directions  𝚲 = diag(λi)  and  𝐐.  The 
volumetric and principal shear logarithmic strains are given by 
𝜃 = log(𝐽) ,
⎜⎜⎜⎛𝜆𝑖
⎟⎟⎟⎞
3⎠
⎝
𝑒𝑖 = log
, 
(22.30.11)
where 
(22.30.12)
𝐽 = 𝜆1𝜆2𝜆3.
𝑛, a value 
is the total Jacobian of the deformation.  Using Equation (22.30.6) with 𝜉S = 𝜉S
𝐹trial  of  the  loading  function  can  be  computed.    The  discrete  counterpart  of  Equation 
(22.30.8) becomes 
𝐹trial − 𝑅s
𝐹trial − 𝐹n > 0
n < 1
𝜉S
AS > 0
⇒ Δ𝜉S
⎫
}
⎬
}
⎭
(22.30.13)
= −(1 − 𝜉S
𝑛 − Δ𝜉S)
𝐹trial − 𝛽Δ𝜉S − min(max(𝐹𝑛, 𝑅s
AS), 𝑅f
AS)
𝐹trial − 𝛽Δ𝜉S − 𝑅f
AS
SA < 0
𝐹trial − 𝑅s
𝐹trial − 𝐹n < 0
n > 0
𝜉S
⎫
}
⎬
}
⎭
⇒ Δ𝜉S = (𝜉S
𝑛 + Δ𝜉𝑆)
𝐹trial − 𝛽Δ𝜉S − min(max(𝐹n, 𝑅f
SA
𝐹trial − 𝛽Δ𝜉S − 𝑅f
SA) , 𝑅s
SA)
.  (22.30.14)
If none of the two conditions to the left are satisfied, set 𝜉S
𝑛, 𝐹𝑛+1 = 𝐹trial 
and compute the stress 𝜎 𝑛+1 using Equations (22.30.1), (22.30.2), (22.30.5), (22.30.10) and 
𝑛.  When  phase  transformation  occurs  according  to  a  condition  to  the  left,  the 
𝜉S = 𝜉S
𝑛+1 = 𝜉S
Material Models 
LS-DYNA Theory Manual 
corresponding equation to the right is solved for Δ𝜉S. If the bulk and shear modulii are 
constant  this  is  an  easy  task.    Otherwise  𝐹trial  as  well  as  𝛽  depends  on  this  parameter 
and makes things a bit more tricky.  We have that  
𝐹trial = 𝐹n
trial (1 +
𝛽 = 𝛽n (1 +
𝐸S − 𝐸A
𝐸n
𝐸S − 𝐸A
𝐸n
Δ𝜉S),
Δ𝜉S) ,
(22.30.15)
where 𝐸S  and  𝐸A  are  Young’s  modulii  for  martensite  and  austenite,  respectively.    The 
subscript  𝑛  is  introduced  for  constant  quantities  evaluated  at  time  𝑡𝑛.    To  simplify  the 
upcoming expressions, these relations are written  
trial + Δ𝐹trialΔ𝜉S,
(22.30.16)
𝐹trial = 𝐹n
𝛽 = 𝛽n + Δ𝛽Δ𝜉S.
Inserting these expressions into Equation (19.30.7) results in  
𝑓 (Δ𝜉S) = Δ𝛽(1 − 𝜉S
𝑛 − 𝐹𝑛
𝑛)(𝐹̃AS
(1 − 𝜉S
𝑛)Δ𝜉S
trial) = 0.
2 + (𝑅f
AS − 𝐹̃AS
𝑛 + (𝛽n − Δ𝐹trial)(1 − 𝜉S
𝑛)) Δ𝜉S +
and 
𝑓 (Δ𝜉S) = Δ𝛽𝜉S
𝑛 − 𝐹𝑛
𝑛(𝐹̃SA
𝜉S
𝑛Δ𝜉S
trial) = 0.
2 + (𝐹̃SA
𝑛 − 𝑅f
SA + (𝛽𝑛 − Δ𝐹trial)𝜉S
𝑛)Δ𝜉S +
respectively, where we have for simplicity set  
𝑛 = min(max(𝐹𝑛, 𝑅s
𝐹̃AS
𝑛 = min(max(𝐹𝑛, 𝑅f
𝐹̃SA
AS) , 𝑅f
SA), 𝑅s
AS) ,
SA).
(22.30.17)
(22.30.18)
(22.30.19)
The  solutions  to  these  equations  are  approximated  with  two  Newton  iterations 
𝑛 + Δ𝜉S))  and  compute 
starting  in  the  point  Δ𝜉S = 0.  Now  set  𝜉S
𝜎 𝑛+1  and  𝐹𝑛+1  according  to  Equations  (22.30.1),  (22.30.2),  (22.30.5),  (22.30.6),  (22.30.10) 
and 𝜉S = 𝜉S
𝑛+1 = min(1, max(0, 𝜉S
𝑛+1. 
22.30.3  Tangent Stiffness Matrix 
An  algorithmic  tangent  stiffness  matrix  relating  a  change  in  true  strain  to  a 
corresponding  change  in  Kirchhoff  stress  is  derived  in  the  following.    Taking  the 
variation of Equation (22.30.2) results in 
δ𝑝 = 𝐾(δ𝜃 − 3𝛼δ𝜉S𝜀L) + δ𝐾(𝜃 − 3𝛼𝜉S𝜀L),
δ𝐭 = 2𝐺(δ𝐞 − δ𝜉S𝜀L𝐧 − 𝜉S𝜀Lδ𝐧) + 2δ𝐺(𝐞 − 𝜉S𝜀L𝐧).
(22.30.20)
(22.30.21)
LS-DYNA Theory Manual 
Material Models 
The variation of the unit vector in Equation (22.30.5) can be written 
δ𝐧 =
‖𝐞‖ + 10−12 (𝐈 − 𝐧 ⊗ 𝐧)δ𝐞,
(22.30.22)
where 𝐈 is the fourth order identity tensor.  For the variation of martensite fraction we 
introduce  the  indicator  parameters  𝐻AS  and  𝐻SA  that  should  give  information  of  the 
probability  of  phase  transformation  occurring  in  the  next  stress  update.    Set  initially 
𝐻AS = 𝐻SA = 0 and change them according to 
AS > 0
𝐹trial − 𝑅s
⎫
}
𝐹trial − 𝐹𝑛 > 0
⎬
}
𝑛 + Δ𝜉S ≤ 1 ⎭
𝜉S
SA < 0
𝐹trial − 𝑅s
⎫
}
𝐹trial − 𝐹𝑛 < 0
⎬
}
𝑛 + Δ𝜉S ≥ 0 ⎭
𝜉S
     ⇒      𝐻AS = 1, 
(22.30.23)
     ⇒      𝐻SA = 1, 
(22.30.24)
using  the  quantities  computed  in  the  previous  stress  update.    For  the  variation  of  the 
martensite fraction we take variations of Equations (22.30.17) and (22.30.18) with  
which results in 
trial = 2𝐺𝐧: δ𝐞 + 3𝛼𝐾δ𝜃,
δ𝐹n
δ𝜉S = γ(2𝐺𝐧: δ𝐞 + 3𝛼𝐾δ𝜃),
where 
𝛾 =
𝑛)𝐻AS
(1 − 𝜉S
𝑛 + (𝛽𝑛 − Δ𝐹𝑛
AS
AS − 𝐹̃
𝑅f
𝑛)
trial)(1 − 𝜉S
𝐹̃
𝑛 − 𝑅f
SA
+
𝑛𝐻SA
𝜉S
SA + (𝛽𝑛 − Δ𝐹𝑛
trial)𝜉S
(22.30.25)
(22.30.26)
. 
(22.30.27)
As can be seen, we use the value of 𝛾 obtained in the previous stress update since 
this is easier to implement and will probably give a good indication of the current value 
of this parameter. 
The variation of the material parameters 𝐾 and 𝐺 results in  
δK = (𝐾S − 𝐾A)δ𝜉S,
δG = (𝐺S − 𝐺A)δ𝜉S,
and, finally, using the identities 
𝐧: δ𝐞 = 𝐧: δ𝛆,
δ𝜃 = 𝐢: δ𝛆,
δ𝛕 = 𝐢δ𝑝 + δ𝐭,
results in 
(22.30.28)
(22.30.29)
(22.30.30)
(22.30.31)
Material Models 
LS-DYNA Theory Manual 
δ𝛕 = {2𝐺 (1 −
𝜉S𝜀L
‖𝐞‖ + 10−12) 𝐈dev
+ 𝐾[1 − 9𝛼2𝐾𝛾𝜀L + 3𝛼𝛾(𝐾S − 𝐾A)(𝜃 − 3𝛼𝜉S𝜀L)]𝐢 ⊗ 𝐢
+ 2γ𝐺(𝐾S − 𝐾A)(𝜃 − 3𝛼𝜉S𝜀L)𝐢 ⊗ 𝐧
+ 6𝛾𝛼𝐾(𝐺S − 𝐺A)(‖𝐞‖ − 𝜉S𝜀L)𝐧 ⊗ 𝐢 
(22.30.32)
+ 2𝐺 [
𝜉S𝜀L
‖𝐞‖ + 10−12 − 2𝐺𝛾𝜀L + 2𝛾(𝐺S − 𝐺A)(‖𝐞‖ − 𝜉S𝜀L)] 𝐧 ⊗ 𝐧
− 6𝐾𝐺𝛼𝛾𝜀L(𝐢 ⊗ 𝐧 + 𝐧 ⊗ 𝐢)} δ𝜀. 
where 𝐈dev is the fourth order deviatoric identity tensor.  In general this tangent is not 
symmetric because of the terms on the second line in the expression above.  We simply 
implementation.  
use  a  symmetrization  of  the  tangent  stiffness  above 
Furthermore, we transform the tangent to a tangent closer related to the one that should 
be used in the LS-DYNA implementation, 
in  the 
𝐂 = 𝐽−1 {2𝐺 (1 −
𝜉S𝜀L
‖𝐞‖ + 10−12) 𝐈dev
+ 𝐾[1 − 9𝛼2𝐾𝛾𝜀L + 3𝛼𝛾(𝐾S − 𝐾A)(𝜃 − 3𝛼𝜉S𝜀L)]𝐢 ⊗ 𝐢
+ 3𝛾𝛼𝐾(𝐺S − 𝐺A)(‖𝐞‖ − 𝜉S𝜀L) − 6𝐾𝐺𝛼𝛾𝜀L))(𝐢 ⊗ 𝐧 + 𝐧 ⊗ 𝐢)
(22.30.33)
+ 2G [
𝜉S𝜀L
‖𝐞‖ + 10−12 − 2𝐺𝛾𝜀L + 2𝛾(𝐺S − 𝐺A)(‖𝐞‖ − 𝜉S𝜀L)] 𝐧 ⊗ 𝐧} δ𝜀.
LS-DYNA Theory Manual 
Material Models 
22.31  Material Model 31:  Slightly Compressible Rubber 
Model 
This model implements a modified form of the hyperelastic constitutive law first 
described in [Kenchington 1988]. 
The strain energy functional, 𝑈, is defined in terms of the input constants as: 
𝑈 = C100𝐼1 + C200𝐼1
          C210𝐼1
2𝐼2 + C010𝐼2 + C020𝐼2
2 + C300𝐼1
3 + C400𝐼1
2 + 𝑓 (𝐽),
4 + C110𝐼1𝐼2 +
(22.31.1)
where  the  strain  invariants  can  be  expressed  in  terms  of  the  deformation  gradient 
matrix, 𝐹𝑖𝑗, and the Green-St.  Venant strain tensor, 𝐸𝑖𝑗: 
𝐽 = ∣𝐹𝑖𝑗∣
𝐼1 = 𝐸𝑖𝑖 
𝐼2 =
𝑖𝑗 𝐸𝑝𝑖𝐸𝑞𝑗.
𝛿𝑝𝑞
2!
(22.31.2)
The derivative of 𝑈 with respect to a component of strain gives the correspond-
ing component of stress 
𝑆𝑖𝑗 =
∂𝑈
∂𝐸𝑖𝑗
,
(22.31.3)
where,  𝑆𝑖𝑗,  is  the  second  Piola-Kirchhoff  stress  tensor  which  is  transformed  into  the 
Cauchy stress tensor: 
𝜎𝑖𝑗 =
𝜌0
𝜕𝑥𝑖
𝜕𝑋𝑘
𝜕𝑥𝑗
𝜕𝑋𝑙
𝑆𝑘𝑙,
(22.31.4)
where 𝜌0 and 𝜌 are the initial and current density, respectively.
Material Models 
LS-DYNA Theory Manual 
22.32  Material Model 32:  Laminated Glass Model 
This  model  is  available  for  modeling  safety  glass.    Safety  glass  is  a  layered 
material of glass bonded to a polymer material which can undergo large strains. 
The glass layers are modeled by isotropic hardening plasticity with failure based 
on  exceeding  a  specified  level  of  plastic  strain.    Glass  is  quite  brittle  and  cannot 
withstand  large  strains  before  failing.    Plastic  strain  was  chosen  for  failure  since  it 
increases monotonically and, therefore, is insensitive to spurious numerical noise in the 
solution.   
The  material  to  which  the  glass  is  bonded  is  assumed  to  stretch  plastically 
without  failure.    The  user  defined  integration  rule  option  must  be  used  with  this 
material.    The  user  defined  rule  specifies  the  thickness  of  the  layers  making  up  the 
safety glass.  Each integration point is flagged with a zero if the layer is glass and with a 
one if the layer is polymer.   
An  iterative  plane  stress  plasticity  algorithm  is  used  to  enforce  the  plane  stress 
condition.
LS-DYNA Theory Manual 
Material Models 
22.33  Material Model 33:  Barlat’s Anisotropic Plasticity 
Model 
This  model  was  developed  by  Barlat,  Lege,  and  Brem  [1991]  for  modeling 
material  behavior  in  forming  processes.    The  finite  element  implementation  of  this 
model is described in detail by Chung and Shah [1992] and is used here. 
The yield function 𝛷 is defined as 
𝛷 = |𝑆1 − 𝑆2|𝑚 + |𝑆2 − 𝑆3|𝑚 + |𝑆3 − 𝑆1|𝑚 = 2𝑚,
(22.33.1)
where  𝜎̅̅̅̅̅  is  the  effective  stress,  and  𝑆𝑖  for  𝑖 = 1, 2, 3  are  the  principal  values  of  the 
symmetric matrix 𝑆𝛼𝛽, 
𝑆𝑥𝑥 =
𝑆𝑦𝑦 =
[𝑐(𝜎𝑥𝑥 − 𝜎𝑦𝑦) − 𝑏(𝜎𝑧𝑧 − 𝜎𝑥𝑥)]
[𝑎(𝜎𝑦𝑦 − 𝜎𝑧𝑧) − 𝑐(𝜎𝑥𝑥 − 𝜎𝑦𝑦)]
[𝑏(𝜎𝑧𝑧 − 𝜎𝑥𝑥) − 𝑎(𝜎𝑦𝑦 − 𝜎𝑧𝑧)]
𝑆𝑧𝑧 =
𝑆𝑦𝑧 = 𝑓 𝜎𝑦𝑧 
𝑆𝑧𝑥 = 𝑔𝜎𝑧𝑥 
𝑆𝑥𝑦 = ℎ𝜎𝑥𝑦.
(22.33.2)
The material constants 𝑎, 𝑏, 𝑐, 𝑓 , 𝑔 and ℎ represent anisotropic properties.  When 
𝑎 = 𝑏 = 𝑐 = 𝑓 = 𝑔 = ℎ = 1, the material is isotropic and the yield surface reduces to the 
Tresca  yield  surface  for  𝑚 = 1  and  von  Mises  yield  surface  for  𝑚 =  2 or 4.  For  face-
centered-cubic  (FCC)  materials  𝑚 = 8  is  recommended  and  for  body-centered-cubic 
(BCC) materials 𝑚 = 6 is used. 
The yield strength of the material is 
𝜎y = 𝑘(1 + 𝜀0)𝑛.
(22.33.3)
Material Models 
LS-DYNA Theory Manual 
22.34  Material Model 34:  Fabric 
The  fabric  model  is  a  variation  on  the  Layered  Orthotropic  Composite  material 
model  (Material  22)  and  is  valid  for  only  3  and  4  node  membrane  elements.    This 
material  model  is  strongly  recommended  for  modeling  airbags  and  seatbelts.    In 
addition  to  being  a  constitutive  model,  this  model  also  invokes  a  special  membrane 
element  formulation  that  is  better  suited  to  the  large  deformations  experienced  by 
fabrics.  For thin fabrics, buckling (wrinkling) can occur with the associated inability of 
the structure to support compressive stresses; a material parameter flag is included for 
this  option.    A  linear  elastic  liner  is  also  included  which  can  be  used  to  reduce  the 
tendency for these material/elements to be crushed when the no-compression option is 
invoked. 
If the airbag material is to be approximated as an isotropic elastic material, then 
only  one  Young’s  modulus  and  Poisson’s  ratio  should  be  defined.    The  elastic 
approximation  is  very  efficient  because  the  local  transformations  to  the  material 
coordinate  system  may  be  skipped.    If  orthotropic  constants  are  defined,  it  is  very 
important to consider the orientation of the local material system and use great care in 
setting up the finite element mesh.  
If  the  reference  configuration  of  the  airbag  is  taken  as  the  folded  configuration, 
the geometrical accuracy of the deployed bag will be affected by both the stretching and 
the  compression  of  elements  during  the  folding  process.    Such  element  distortions  are 
very difficult to avoid in a folded bag.  By reading in a reference configuration such as 
the  final  unstretched  configuration  of  a  deployed  bag,  any  distortions  in  the  initial 
geometry of the folded bag will have no effect on the final geometry of the inflated bag.  
This is because the stresses depend only on the deformation gradient matrix: 
𝐹𝑖𝑗 =
𝜕𝑥𝑖
𝜕𝑋𝑗
,
(22.34.1)
where the choice of 𝑋𝑗 may coincide with the folded or unfold configurations.  It is this 
unfolded configuration which may  be specified here.  When the reference geometry is 
used then the no-compression option should be active.  With the reference geometry it 
is possible to shrink the airbag and then perform the inflation.  Although the elements 
in  the  shrunken  bag  are  very  small,  the  time  step  can  be  based  on  the  reference 
geometry so a very reasonable time step size is obtained.  The reference geometry based 
time step size is optional in the input. 
The  parameters  fabric  leakage  coefficient, FLC,  fabric  area  coefficient,  FAC,  and 
effective leakage area, ELA, for the fabric in contact with the structure are optional for 
the  Wang-Nefske  and  hybrid  inflation  models.    It  is  possible  for  the  airbag  to  be 
constructed  of  multiple  fabrics  having  different  values  of  porosity  and  permeability.
LS-DYNA Theory Manual 
Material Models 
The gas leakage through the airbag fabric then requires an accurate determination of the 
areas by part ID available for leakage.  The leakage area may change over time due to 
stretching of the airbag fabric or blockage when the outer surface of the bag is in contact 
with  the  structure.    LS-DYNA  can  check  the  interaction  of  the  bag  with  the  structure 
and split the areas into regions that are blocked and unblocked depending on whether 
the regions are in contact or not, respectively.  Typically, the parameters, FLC and FAC, 
must  be  determined  experimentally  and  their  variation  with  time  and  pressure  are 
optional inputs that allow for maximum modeling flexibility.
Material Models 
LS-DYNA Theory Manual 
22.35  Material Model 35:  Kinematic/Isotropic Plastic Green-
Naghdi Rate 
The  reader  interested  in  an  detailed  discussion  of  the  relative  merits  of  various 
stress  rates,  especially  Jaumann  [1911]  and  Green-Naghdi  [1965],  is  urged  to  read  the 
work of Johnson and Bammann [1984].  A mathematical description of these two stress 
rates, and how they are implemented in LS-DYNA, is given in the section entitled Stress 
Update Overview in this manual. 
In  the  cited  work  by  Johnson  and  Bammann,  they  conclude  that  the  Green-
Naghdi stress rate is to be preferred over all other proposed stress rates, including the 
most widely used Jaumann rate, because the Green-Naghdi stress rate is based on the 
notions  of 
  However, 
invariance  under  superimposed  rigid-body  motions. 
implementation  of  the  Green-Naghdi  stress  rate  comes  at  a  significant  computational 
cost compared to the Jaumann stress rate, e.g., see the discussion in this manual in the 
section entitled Green-Naghdi Stress Rate. 
Perhaps  more  importantly,  in  practical  applications  there  is  little  if  any  noted 
difference  in  the  results  generated  using  either  Jaumann  or  Green-Naghdi  stress  rate.  
This  is  in  part  due  to  the  fact  that  the  Jaumann  stress  rate  only  produces  erroneous 
results2 when linear kinematic hardening is used; the results for isotropic hardening are 
not  affected  by  the  choice  of  either  of  these  two  stress  rates.    Also  in  practical 
applications, the shear strains are rather small, compared to the extensional strains, and 
if they are not small it is usually the case that the material description, i.e., constitutive 
model, is not valid for such large shear strains.
2  The  results  of  a  simple  shear  simulation,  monotonically  increasing  shear  deformation,  produce 
sinusoidal stress response.
LS-DYNA Theory Manual 
Material Models 
22.36  Material Model 36:  Barlat’s 3-Parameter Plasticity 
Model 
Material model 36 in LS-DYNA aims at modeling sheets with anisotropy under 
plane stress conditions.  It allows the use of the Lankford parameters for the definition 
of the anisotropic yield surface.  The yield condition can be written 
𝑓 (𝛔, 𝜀p) = 𝜎eff(𝜎11, 𝜎22, 𝜎12) − 𝜎Y(𝜀p) ≤ 0,
(22.36.1)
where 
𝜎eff(𝜎11, 𝜎22, 𝜎12) = (
𝐾1 = 𝐾1(𝜎11, 𝜎22, 𝜎12) =
|𝐾1 + 𝐾2|𝑚 +
𝜎11 + ℎ𝜎22
|𝐾1 − 𝐾2|𝑚 +
1/𝑚
|2𝐾2|𝑚)
(22.36.2)
𝐾2 = 𝐾2(𝜎11, 𝜎22, 𝜎12) = √(
𝜎11 − ℎ𝜎22
)
2 ,
+ 𝑝2𝜎12
and the hardening of the yield surface is either linear, exponential or determined by a 
load curve.  In the above, the stress components 𝜎11, 𝜎22 and 𝜎12 are with respect to the 
material  coordinate  system  and  𝜀p  denotes  the  effective  plastic  strain.    The  material 
parameters 𝑎, 𝑐, ℎ and 𝑝 can be determined from the Lankford parameters as described 
in  the  LS-DYNA Keyword  User’s Manual  [Hallquist  2003].    The  Lankford  parameters, 
or  R-values,  are  defined  as  the  ratio  of  instantaneous  width  change  to  instantaneous 
thickness  change.    That  is,  assume  that  the  width  𝑊  and  thickness  𝑇  are  measured  as 
function of strain.  Then the corresponding R-value is given by 
𝑅 =
𝑑𝑊
𝑑𝜀
𝑑𝑇
𝑑𝜀
/𝑊
/𝑇
. 
The gradient of the yield surface is denoted  
∂𝑓
∂𝛔
(𝛔) =
∂𝑓
∂𝜎11
∂𝑓
∂𝜎22
∂𝑓
∂𝜎12
⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛
⎝
where 
LS-DYNA Draft 
(𝛔)
(𝛔)
(𝛔)
⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞
⎠
𝜕𝑓
𝜕𝜎11
𝜕𝑓
𝜕𝜎22
𝜕𝑓
𝜕𝜎12
(𝜎11, 𝜎22, 𝜎12)
(𝜎11, 𝜎22, 𝜎12)
(𝜎11, 𝜎22, 𝜎12)
, 
⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞
⎠
=
⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛
⎝
Material Models 
LS-DYNA Theory Manual 
(𝜎11, 𝜎22, 𝜎12) =
𝜎eff(𝜎11, 𝜎22, 𝜎12)1−𝑚
⋅
∂𝜎eff
∂𝜎11
(𝜎11, 𝜎22, 𝜎12) =
𝜕𝑓
𝜕𝜎11
    {𝑎(𝐾1 − 𝐾2)|𝐾1 − 𝐾2|𝑚−2 (
        𝑎(𝐾1 + 𝐾2)|𝐾1 + 𝐾2|𝑚−2 (
        𝑐2𝑚𝐾2
𝑚−1 𝜎11 − ℎ𝜎22
} ,
4𝐾2
) +
−
𝜎11 − ℎ𝜎22
4𝐾2
𝜎11 − ℎ𝜎22
4𝐾2
+
) +
(22.36.4) 
(𝜎11, 𝜎22, 𝜎12) =
𝜎eff(𝜎11, 𝜎22, 𝜎12)1−𝑚
ℎ ⋅
𝜕𝜎eff
𝜕𝜎22
(𝜎11, 𝜎22, 𝜎12) =
𝜕𝑓
𝜕𝜎22
    {𝑎(𝐾1 − 𝐾2)|𝐾1 − 𝐾2|𝑚−2 (
        𝑎(𝐾1 + 𝐾2)|𝐾1 + 𝐾2|𝑚−2 (
) +
+
𝜎11 − ℎ𝜎22
4𝐾2
𝜎11 − ℎ𝜎22
4𝐾2
−
) −
(22.36.5) 
        𝑐2𝑚𝐾2
𝑚−1 𝜎11 − ℎ𝜎22
} ,
4𝐾2
and 
(𝜎11, 𝜎22, 𝜎12) =
𝜕𝑓
𝜕𝜎12
    {−𝑎(𝐾1 − 𝐾2)|𝐾1 − 𝐾2|𝑚−2 + 𝑎(𝐾1 + 𝐾2)|𝐾1 + 𝐾2|𝑚−2 + 𝑐2𝑚𝐾2
𝜎eff(𝜎11, 𝜎22, 𝜎12)1−𝑚
(𝜎11, 𝜎22, 𝜎12) =
𝜕𝜎eff
𝜕𝜎12
𝑝2𝜎12
𝐾2
𝑚−1}.
⋅
(22.36.6)
22.36.1  Material Tangent Stiffness 
Since the plastic model is associative, the general expression for tangent relating 
the  total  strain  rate  to  total  stress  rate  can  be  found  in  standard  textbooks.    Since  this 
situation is rather special we derive it here for the plane stress model presented in the 
previous section.  The elastic stress-strain relation can be written 
1 − 𝜈
𝛔̇ =
⎟⎟⎟⎟⎟⎟⎟⎟⎞
𝜎̇11
𝜎̇22
𝜎̇12
𝜎̇23
𝜎̇13⎠
⎜⎜⎜⎜⎜⎜⎜⎜⎛
⎝
=
1 − ν2
⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛
⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞
1 − 𝜈
1 − 𝜈
⎝
= 𝐂ps(𝛆̇ − 𝛆̇p). 
2 ⎠
𝜀̇11 − 𝜀̇11
𝜀̇22 − 𝜀̇22
p )
2(𝜀̇12 − 𝜀̇12
p )
2(𝜀̇23 − 𝜀̇23
p )⎠
2(𝜀̇13 − 𝜀̇13
⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞
⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛
⎝
(22.36.7)
where  𝐸  is  the  Young’s  modulus,  𝜈  is  the  Poisson’s  ratio  and  𝐂ps  denotes  the  plane 
stress elastic tangential stiffness matrix.  The associative flow rule for the plastic strain 
can be written
LS-DYNA Theory Manual 
Material Models 
and the consistency condition results in  
𝛆̇p = λ̇
∂𝑓
∂𝛔
,
∂𝑓 T
∂𝛔
𝛔̇ +
∂𝑓
∂𝜀p
𝛆̇p = 0.
(22.36.8)
(22.36.9)
For algorithmic consistency, the effective plastic strain rate is defined as  𝜀̇p = 𝜆̇. 
∂𝑓
∂𝛔  and  using  Equation  (22.36.8)  and  Equation 
Multiplying  Equation  (22.36.7)  with 
(22.36.9) gives 
𝐂ps𝛆̇
∂𝑓
∂𝛔
𝐂ps ∂𝑓
∂𝛔
. 
−
∂𝑓
∂𝜀p
λ̇ =
∂𝑓
∂𝛔
Inserting 
𝛆̇p =
∂𝑓
∂𝛔
into Equation (22.36.7) results in  
𝐂ps𝛆̇
∂𝑓
∂𝛔
𝐂ps ∂𝑓
∂𝛔
−
∂𝑓
∂𝜀p
∂𝑓
∂𝛔
, 
𝐂ps −
𝛔̇ =
⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛
⎝
}
} {𝐂ps ∂𝑓
∂𝛔
{𝐂ps ∂𝑓
∂𝛔
𝐂ps ∂𝑓
∂𝛔
∂𝑓
∂𝛔
−
∂𝑓
∂𝜀p ⎠
⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞
(22.36.10)
(22.36.11)
𝛆̇. 
(22.36.12)
To get the elastic-plastic tangent stiffness tensor in the element coordinate system 
it needs to be transformed back.  Since the elastic tangential stiffness tensor is isotropic 
with respect to the axis of rotation, the plastic tangent stiffness tensor can be written  
ps
𝐂plastic
=
𝐂ps −
⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛
⎝
{𝐐𝐂ps ∂𝑓
∂𝛔
𝐂ps ∂𝑓
∂𝛔
∂𝑓
∂𝛔
} {𝐐𝐂ps ∂𝑓
∂𝛔
}
−
∂𝑓
∂𝜀p ⎠
⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞
, 
(22.36.13)
where 𝐐 is the rotation matrix in Voigt form.
Material Models 
LS-DYNA Theory Manual 
𝜎22 
𝒏(𝑅𝜑)  𝜕𝑓
𝜕𝝈
𝒏(𝑅45)
𝜎𝑌
𝜕𝑓
𝜕𝝈
𝜕𝑓
𝜕𝝈
𝒏(𝑅90) 
𝑓 (𝝈, 𝜀𝑝) ≤ 0 
𝜎𝑌(𝜀𝑝) 
𝛼00, 𝛼45, 𝛼90
changes  
𝒏(𝑅00) 
𝜕𝑓
𝜕𝝈
𝜎11
90(𝜀𝑝) 
𝜎𝑌
45(𝜀𝑝) 
𝜎𝑌
00(𝜀𝑝) 
𝜎𝑌
𝜀𝑝
22-1  Plastic  flow  direction  (left)  and  hardening  (right)  illustrated  for 
variable R-values and hardening.  Changes in 𝛼00, 𝛼45 and 𝛼90 come from 
22.36.2  Load curves in different directions 
A project by Fleischer et.al.  [2007] resulted in the option HR = 7, see *MAT_036 in LS-
DYNA  Keyword  User’s  Manual,  which  allows  for  specification  of  different  hardening 
curves in the three directions corresponding to 0, 45 and 90 degrees.  In addition, the R-
values  in  these  directions  can  be  specified  as  functions  of  plastic  strains,  both  features 
make  up  an  interesting  extension  to  the  standard  form  of  the  material  model.    This 
section  is  devoted  to  the  theory  of  the  hardening  option  while  the  theory  for  the  R-
values follows in the next section.  
An introductory remark 
22.36.2.1 
This  material  typically  fits  three  Lankford  parameters  and  the  yield  stress  in  the  00 
direction.    This  fit  will  result  in  a  non-intuitive  effective  stress-strain  relationship  for 
uniaxial  tension  in  other  directions.    To  explain  this  we  assume  that  we  pull  in  the  𝜑 
direction  giving  a  uniaxial  stress  value  of  𝜎𝜑  and  a  corresponding  plastic  strain 
𝑝 . The relation between the stress value 𝜎𝜑 and effective stress 𝜎eff is given 
component 𝜀𝜑
by  
𝜎eff = 𝑘𝜑𝜎𝜑 
where 𝑘𝜑 = 1 if  𝜑 = 0 but not in general.  The plastic  work relation, which defines the 
effective  plastic  strain  for  the  current  material,  gives  the  following  expression  for  the 
effective plastic strain  
𝜀𝑝 =
𝑝 𝜎𝜑
𝜀𝜑
𝜎eff
. 
This  means  that  there  is  a  relationship  with  a  stress-strain  hardening  curve  using  the 
effective stress and strain and a corresponding stress-strain hardening curve using the 
actual stress and strain values.  Assume that a test reveals that the hardening is given by 
the curve
LS-DYNA Theory Manual 
Material Models 
𝜎𝜑 = 𝜎𝜑(𝜀𝜑
𝑝 ) 
and we want to determine the hardening curve used by LS-DYNA 
𝜎eff = 𝜎eff(𝜀𝑝), 
then using the relationships above yields 
𝜎eff(𝜀𝑝) = 𝑘𝜑𝜎𝜑(𝑘𝜑𝜀𝑝). 
Consequently  a  user  input  hardening  curve  must  internally  be  transformed  to  an 
effective hardening curve to be used in the material model to get the desired behavior.  
Still, the effective plastic strain is not going to be equal to the plastic strain component in 
the  tensile  direction  and  validation  of  the  hardening  behavior  is  not  straightforward.  
Therefore we introduce a new effective plastic strain 𝜀𝑝̃ with evolution given by 
𝑑𝜀𝑝̃
𝑑𝑡 = 𝑘𝜑
𝑑𝜀𝑝
𝑑𝑡  
that  can  be  used  to  verify  the  hardening  relationship.    This  is  actually  the  von  Mises 
plastic  strain  in  the  work  hardening  sense  and  is  output  to  the  d3plot  database  as 
history variable #2 for post-processing. 
The model 
22.36.2.2 
The load curve hardening option can be generalized to allow different hardening curves 
in  the  00,  45  and  90  directions,  as  well  as  balanced  biaxial  and  shear  loading.    To  this 
end we let the yield value be given as a convex combination of the hardening curves in 
each direction as 
𝜎𝑌(𝝈, 𝜀𝑝) = 𝛼00𝜎𝑌
00(𝜀𝑝) +   𝛼45𝜎𝑌
45(𝜀𝑝) + 𝛼90𝜎𝑌
90(𝜀𝑝) + 𝛼bi𝜎𝑌
bi(𝜀𝑝) + 𝛼sh𝜎𝑌
sh(𝜀𝑝) 
00(𝜀𝑝)  is  the  user  defined  hardening  curve  in  direction  00,  and  the  others  are 
where  𝜎𝑌
the internal hardening curves in the other directions . The convex parameters must fulfill 
0 ≤ 𝛼00 ≤ 1,  0 ≤ 𝛼45 ≤ 1,  0 ≤ 𝛼90 ≤ 1, 0 ≤ 𝛼bi ≤ 1, 0 ≤ 𝛼sh ≤ 1, 
𝛼00 + 𝛼45 + 𝛼90 + 𝛼bi + 𝛼sh = 1, 
and  depend  on  the  stress  state.    Furthermore  𝛼00 = 1  must  mean  that  the  stress  is 
uniaxial and is directed in the 00 direction, and that the same thing holds for the other 
directions.  To accomplish this we reason as follows. 
Let 𝜎̂𝑖𝑗 be the normalized in-plane stress components, i.e.,  
𝜎̂𝑖𝑗 =
𝜎𝑖𝑗
2 +𝜎22
√𝜎11
2 +2𝜎12
and  let  𝜎  be  the  largest  eigenvalue  to  this  matrix  and  𝑞𝑖  the  associated  eigenvector 
components.    Furthermore  we  define  𝜎𝑣 = (𝜎̂11 + 𝜎̂22)/2  as  the  normalized  volumetric 
stress and 𝜎𝑑 = √(𝜎̂11−𝜎̂22)2
𝜎𝑑 ≤ 1/√2 and 
2   the normalized shear stress, and make a note that 0 ≤
+ 𝜎̂12
𝜎𝑑 = 0 → biaxial stress state 
𝜎𝑑 = 1/2 → uniaxial stress state 
𝜎𝑑 = 1/√2 → shear stress state. 
2 is the fraction of stress that is volumetric and 𝑏 = 𝜎 2 an indicator of uniaxial 
If 𝑎 = 2𝜎𝑣
stress  state,  then    𝑐 = 𝑎(1 − 4{𝑏 − 1/2}2)  is  a  normalized  measure  that  indicates  when
Material Models 
LS-DYNA Theory Manual 
2(1 − 𝑞1
the  stress  is  deviatoric/uniaxial  or  volumetric.    That  is,  𝑐 = 0  means  that  the  stress  is 
deviatoric or uniaxial and 𝑐 = 1 means that it is volumetric. 
2) be the fraction of the eigenvector 𝑞𝑖 that points in the 00 or 90 
Now, let 𝑞 = 4𝑞1
direction.  That is, 𝑞 = 1 means that the eigenvector points in the 45 direction and 𝑞 = 0 
means  that  it  is  pointing  in  either  the  00  or  90  direction.    Moreover,  the  same  way  of 
reasoning is valid for the eigenvector associated to the smallest eigenvalue. 
To  determine  in  which  direction  of  00  or  90  a  certain  eigenvector  is  pointing  we 
2), and deduce that 𝑑 = 1 means that the eigenvector 𝑞𝑖 
introduce 𝑑 = 𝑏𝑞1
points in the 00 direction and 𝑑 = 0 means that it is pointing in the 90 direction. 
 We are now ready to give partial expressions for the three uniaxial convex parameters 
2 + (1 − 𝑏)(1 − 𝑞1
𝛼̃00 = (1 − 𝑐)𝑑(1 − 𝑞) + 𝑐/4 
𝛼̃45 = (1 − 𝑐)𝑞 + 𝑐/2 
𝛼̃00 = (1 − 𝑐)(1 − 𝑑)(1 − 𝑞) + 𝑐/4 
and these are completed by means of adding the biaxial and shear parts 
2) 
2 − 1) 
𝛼bi = max (0,1 − 4𝜎𝑑
𝛼sh = max (0,4𝜎𝑑
𝛼00 = 𝛼̃00(1 − 𝛼bi − 𝛼sh) 
𝛼45 = 𝛼̃45(1 − 𝛼bi − 𝛼sh) 
𝛼90 = 𝛼̃90(1 − 𝛼bi − 𝛼sh) 
This  set  of  parameters  fulfills  the  requirements  mentioned  above  and  allows  for  a 
decent expression for a directional dependent yield stress.  
In  the  consistency  condition  we  do  not  consider  the  derivatives  of  the  convex 
parameters  with  respect  to  the  stress,  as  we  assume  that  these  will  not  have  a  major 
impact on convergence. 
22.36.3  Variable Lankford parameters 
The  R-values  are  supposed  to  be  variable  with  deformation,  and  we  let  𝑅00(𝜀𝑝), 
𝑅45(𝜀𝑝) and  𝑅90(𝜀𝑝)  be  the  internal  load  curves  that  are  transformed  from  the  ones 
given by the user.  Then we define the directional dependent R-value according to 
𝑅(𝝈, 𝜀𝑝) = 𝛼00𝑅00(𝜀𝑝) +   𝛼45𝑅45(𝜀𝑝) + 𝛼90𝑅90(𝜀𝑝) 
using  the  same  set  of  convex  parameters  as  in  the  previous  section.    A  generalized 
relation for the R-value in terms of the stress can be given as 
(𝜎̂22 + {𝜎̂11 + 𝜎̂22}𝑅)𝑛1 + (𝜎̂11 + {𝜎̂11 + 𝜎̂22}𝑅)𝑛2 − 𝜎̂12𝑛4 = 0, 
where 𝜎̂𝑖𝑗  are  the  normalized  stress  components,  𝑛𝑖  is  the  direction of plastic  flow  and 
where we have suppressed the dependence of stress and plastic strain in 𝑅. By setting  
∆𝑛1 = 𝑛1 −
𝜕𝑓
𝜕𝜎11
,  ∆𝑛2 = 𝑛2 −
𝜕𝑓
𝜕𝜎22
,  ∆𝑛4 = 𝑛4 −
𝜕𝑓
𝜕𝜎12
and 
∆𝑅 = 𝑅(𝜀𝑝) − 𝑅(0)  
we can simplify this equation as 
(𝜎̂22 + {𝜎̂11 + 𝜎̂22}𝑅)∆𝑛1 + (𝜎̂11 + {𝜎̂11 + 𝜎̂22}𝑅)∆𝑛2 − 𝜎̂12∆𝑛4 = 
−(
𝜕𝑓
𝜕𝜎11
+
𝜕𝑓
𝜕𝜎22
){𝜎̂11 + 𝜎̂22}∆𝑅
LS-DYNA Theory Manual 
Material Models 
assuming that the relation already holds for the yield surface normal and R-value in the 
reference configuration. 
This equation is complemented with a consistency condition of the plastic flow 
𝜎̂11∆𝑛1 + 𝜎̂22∆𝑛2 + 𝜎̂12∆𝑛4 = 0. 
These two equations are linearly independent if and only if 
{𝜎̂11 + 𝜎̂22}√(𝜎̂11−𝜎̂22)2
+ 𝜎̂12
2 ≠ 0 
and then the equation 
−𝜎̂12∆𝑛1 + 𝜎̂12∆𝑛2 + (𝜎̂11 − 𝜎̂22)∆𝑛4 = 0 
can be used to complement the previous two.  This defines a system of equations that 
can be used to solve in least square sense for the perturbation ∆𝑛𝑖 of  the yield surface 
normal  to  get  the  R-value  of  interest.    To  avoid  numerical  problems  and  make  the 
perturbation  continuous  with  respect  to  the  stress,  the  right  hand  side  of  the  first 
equation is changed to 
𝜕𝑓
𝜕𝜎11
){𝜎̂11 + 𝜎̂22}((𝜎̂11 − 𝜎̂22)2 + 4𝜎̂12
2 )∆𝑅. 
𝜕𝑓
𝜕𝜎22
−(
+
This results in a non-associated flow rule, meaning that the plastic flow is not in the 
direction of the yield surface normal.  Again, we don’t take any special measures into 
account for the stress return algorithm as we believe that the perturbation of the normal 
is small enough not to deteriorate convergence.  In figure 22-1 the plastic flow direction 
is illustrated as function of the stress on the yield surface.
Material Models 
LS-DYNA Theory Manual 
22.37  Material Model 37:  Transversely Anisotropic Elastic-
Plastic 
This  fully  iterative  plasticity  model  is  available  only  for  shell  elements.    The 
input  parameters  for  this  model  are:  Young’s  modulus  𝐸;  Poisson’s  ratio  𝜐;  the  yield 
stress; the tangent modulus 𝐸t; and the anisotropic hardening parameter 𝑅.  
Consider  Cartesian  reference  axes  which  are  parallel  to  the  three  symmetry 
planes of anisotropic behavior.  Then the yield function suggested by Hill [1948] can be 
written 
F(𝜎22 − 𝜎33)2 + G(𝜎33 − 𝜎11)2 + H(𝜎11 − 𝜎22)2 + 2L𝜎23
where  𝜎y1,  𝜎y2,  and  𝜎y3,  are  the  tensile  yield  stresses  and  𝜎y12,  𝜎y23,  and  𝜎y31  are  the 
shear yield stresses.  The constants F, G, H, L, M, and N are related to the yield stress by 
2 − 1 = 0,(22.37.1)
2 + 2M𝜎31
2 + 2N𝜎12
2L =
2M =
2N =
2F =
2G =
2H =
𝜎y23
2  
𝜎y31
2  
𝜎y12
2 +
𝜎y2
2 +
𝜎y3
2 +
𝜎y1
2 −
𝜎y3
2 −
𝜎y1
2 −
𝜎y2
2  
𝜎y1
2  
𝜎y2
2  . 
𝜎y3
The isotropic case of von Mises plasticity can be recovered by setting 
and  
F = G = H =
L = M = N =
2,
2𝜎y
2.
2𝜎y
(22.37.2)
(22.37.3)
(22.37.4)
For the particular case of transverse anisotropy, where properties do not vary in 
the 𝑥1 − 𝑥2 plane, the following relations hold:
LS-DYNA Theory Manual 
Material Models 
F = 2G =
2H =
N =
2 −
𝜎y
2 −
𝜎y
𝜎y3
2  
𝜎y3
2 , 
𝜎y3
where it has been assumed that 𝜎y1 = 𝜎y2 = 𝜎y. 
Letting K =
𝜎y
𝜎y3
, the yield criterion can be written 
𝑭(𝛔) = 𝜎e = 𝜎y,
where 
𝐹(𝛔) ≡ [𝜎11
2 + 𝜎22
2 + K2𝜎33
2 − K2𝜎33(𝜎11 + 𝜎22) − (2 − K2)𝜎11𝜎22
+2L𝜎y
2(𝜎23
2 + 𝜎31
2 ) + 2 (2 −
2 ]
K2) 𝜎12
2⁄
.
(22.37.5)
(22.37.6)
(22.37.7)
The  rate  of  plastic  strain  is  assumed  to  be  normal  to  the  yield  surface  so  𝜀̇𝑖𝑗
p  is 
found from 
p = λ
𝜀̇𝑖𝑗
∂𝐹
∂𝜎𝑖𝑗
.
(22.37.8)
Now consider the case of plane stress, where 𝜎33 = 0.  Also, define the anisotropy 
input  parameter  𝑅  as  the  ratio  of  the  in-plane  plastic  strain  rate  to  the  out-of-plane 
plastic strain rate: 
It then follows that 
𝑅 =
𝜀̇22
p .
𝜀̇33
𝑅 =
K2 − 1.
(22.37.9)
(22.37.10)
Using the plane stress assumption and the definition of 𝑅, the yield function may 
now be written  
F(𝛔) = [𝜎11
2 + 𝜎22
2 −
2R
R + 1
𝜎11𝜎22 + 2
2R + 1
R + 1
2⁄
.
2 ]
𝜎12
(22.37.11)
Material Models 
LS-DYNA Theory Manual 
22.38  Material Model 38:  Blatz-Ko Compressible Foam 
𝑊(𝐼1, 𝐼2, 𝐼3) =
𝐼2
𝐼3
where 𝜇 is the shear modulus and 𝐼1, 𝐼2, and 𝐼3 are the strain invariants.  Blatz and Ko 
[1962]  suggested  this  form  for  a  47  percent  volume  polyurethane  foam  rubber  with  a 
Poisson’s ratio of  0.25.  The second Piola-Kirchhoff stresses are given as  
+ 2√𝐼3 − 5),
(22.38.1)
(
𝑆𝑖𝑗 = 𝜇 [(𝐼𝛿𝑖𝑗 − 𝐺𝑖𝑗)
𝐼3
+ (√𝐼3 −
) 𝐺𝑖𝑗],
𝐼2
𝐼3
(22.38.2)
where 𝐺𝑖𝑗 =
stress tensor: 
𝜕𝑥𝑘
𝜕𝑋𝑖
𝜕𝑥𝑘
𝜕𝑋𝑗
, 𝐺𝑖𝑗 =
𝜕𝑋𝑖
𝜕𝑥𝑘
𝜕𝑋𝑗
𝜕𝑥𝑘
, after determining 𝑆𝑖𝑗, it is transformed into the Cauchy 
σ𝑖𝑗 =
𝜌0
𝜕𝑥𝑖
𝜕𝑋𝑘
𝜕𝑥𝑗
𝜕𝑋𝑙
𝑆𝑘𝑙,
(22.38.3)
where 𝜌0 and 𝜌 are the initial and current density, respectively.
LS-DYNA Theory Manual 
Material Models 
22.39  Material Model 39:  Transversely Anisotropic Elastic-
Plastic With FLD 
See  Material  Model  37  for  the  similar  model  theoretical  basis.    The  first  history 
variable is the maximum strain ratio defined by: 
𝜀majorworkpiece
εmajorfld
(22.39.1)
corresponding to 𝜀minorworkpiece.  This history variable replaces the effective plastic strain 
in  the  output.    Plastic  strains  can  still  be  obtained  but  one  additional  history  variable 
must be written into the D3PLOT database. 
The strains on which these calculations are based are integrated in time from the 
strain rates: 
mjr = 0
mjr
Plane Strain
mnr
mjr
mnr
mjr
Draw
Stretch
80
70
60
50
40
30
20
10
%
-50
-40
-30
-20
-10
10
20
30
40
50
% Minor Strain
Figure 22.39.1.  Flow limit diagram. 
𝑛+1 = 𝜀𝑖𝑗
𝜀𝑖𝑗
𝑛 + 𝜀𝑖𝑗
∇𝑛+1
2⁄
Δ𝑡𝑛+1
2⁄ ,
(22.39.2) 
and are stored as history variables.  The resulting strain measure is logarithmic.
Material Models 
LS-DYNA Theory Manual 
22.40  Material Model 42:  Planar Anisotropic Plasticity Model 
This  model is built into LS-DYNA as a user  material model for modeling plane 
stress  anisotropic  plasticity  in  shells.    Please  note  that only  three  cards  are  input  here.  
The orthotropic angles must be defined later as for all materials of this type.  This model 
is currently not vectorized. 
This  is  an  implementation  of  an  anisotropic  plasticity  model  for  plane  stress 
where the flow rule, see Material Type 37, simplifies to: 
𝐹(𝜎22)2 + 𝐺(𝜎11)2 + 𝐻(𝜎11 − 𝜎22)2 + 2𝑁𝜎12
2 − 1 = 0.
(22.40.1)
The  anisotropic  parameters  R00,  R45,  and  R90  are  defined  in  terms  of  𝐹,  𝐺,  𝐻, 
and 𝑁 as [Hill, 1989]: 
2𝑅00 =
2𝑅45 =
2𝑅90 =
,
2𝑁
(𝐹 + 𝐺)
.
− 1, 
(22.40.2) 
The yield function for this model is given as: 
𝜎y = 𝐴𝜀𝑚𝜀̇𝑛.
(22.40.3)
To avoid numerical problems the minimum strain rate, 𝜀̇min must be defined and 
the initial yield stress 𝜎0 is calculated as 
𝜎0 = 𝐴𝜀0
𝑚𝜀̇min
𝑛 = 𝐸𝜀0,
𝜀0 = (
𝑚−1
.
𝑛 )
𝐴𝜀̇min
(22.40.4) 
(22.40.5)
LS-DYNA Theory Manual 
Material Models 
22.41  Material Model 51:  Temperature and Rate Dependent 
Plasticity 
The kinematics associated with the model are discussed in references [Hill 1948, 
Bammann  and  Aifantis  1987,  Bammann  1989].    The  description  below  is  taken  nearly 
verbatim from Bammann [Hill 1948]. 
With the assumption of linear elasticity we can write, 
= 𝜆tr(𝐃e)𝟏 + 2𝜇𝐃e,
where, the Cauchy stress 𝛔 is convected with the elastic spin 𝐖e as, 
= 𝛔̇ − 𝐖e𝛔 + 𝛔𝐖e.
(22.41.1)
(22.41.2)
This  is  equivalent  to  writing  the  constitutive  model  with  respect  to  a  set  of 
directors whose direction is defined by the plastic deformation [Bammann and Aifantis 
1987,  Bammann  and  Johnson  1987].    Decomposing  both  the  skew  symmetric  and 
symmetric  parts  of  the  velocity  gradient  into  elastic  and  plastic  parts  we  write  for  the 
elastic stretching 𝐃e and the elastic spin 𝐖e, 
𝐃e = 𝐃 − 𝐃p − 𝐃th, 𝐖e = 𝐖 = 𝐖p.
(22.41.3)
Within this structure it is now necessary to prescribe an equation for the plastic 
spin 𝐖p in addition to the normally prescribed flow rule for 𝐃p and the stretching due 
to the thermal expansion 𝐃th.  As proposed, we assume a flow rule of the form, 
𝐃p = 𝑓 (𝑇) sinh [
|𝛏| − 𝜅 − 𝑌(𝑇)
𝑉(𝑇)
]
𝛏′
∣𝛏′∣
,
(22.41.4)
where 𝑇 is the temperate, 𝜅 is the scalar hardening variable, 𝛏′ is the difference between 
the deviatoric Cauchy stress 𝛔′ and the tensor variable 𝛂′, 
𝛏′ = 𝛔′ − 𝛂′,
(22.41.5)
and  𝑓 (𝑇),  𝑌(𝑇),  𝑉(𝑇)  are  scalar  functions  whose  specific  dependence  upon  the 
temperature  is  given  below.    Assuming  isotropic  thermal  expansion,  and  introducing 
the expansion coefficient 𝐴̇, the thermal stretching can be written, 
𝐃th = 𝐴̇𝑇̇𝟏.
(22.41.6)
The  evolution  of  the  internal  variables  𝛼  and  𝜅  are  prescribed  in  a  hardening 
minus recovery format as, 
= ℎ(𝑇)𝐃p − [𝑟d (T) ∣𝐃p∣ + 𝑟s(𝑇)] |𝛂|𝛂,
(22.41.7)
Material Models 
LS-DYNA Theory Manual 
𝜅̇ = 𝐻(𝑇)𝐃p − [𝑅d(𝑇) ∣𝐃p∣ − 𝑅s(𝑇)]𝜅2,
(22.41.8) 
where  ℎ  and  𝐻  are  the  hardening  moduli,  𝑟𝑠(𝑇)  and  𝑅s(𝑇)  are  scalar  functions 
describing  the  diffusion  controlled  ‘static’  or  ‘thermal’  recovery,  and  𝑟d(𝑇)  and  𝑅d(𝑇) 
are the functions describing dynamic recovery.   
If  we  assume  that  𝐖p = 0,  we  recover  the  Jaumann  stress  rate  which  results  in 
the prediction of an oscillatory shear stress response in simple shear when coupled with 
a Prager kinematic hardening assumption [Johnson and Bammann 1984].  Alternatively 
we can choose, 
𝐖p = 𝐑T𝐔̇ 𝐔−1𝐑,
(22.41.9)
which  recovers  the  Green-Naghdi  rate  of  Cauchy  stress  and  has  been  shown  to  be 
equivalent  to  Mandel’s  isoclinic  state  [Bammann  and  Aifantis  1987].    The  model 
employing  this  rate  allows  a  reasonable  prediction  of  directional  softening  for  some 
materials  but  in  general  under-predicts  the  softening  and  does  not  accurately  predict 
the axial stresses which occur in the torsion of the thin walled tube.   
The  final  equation  necessary  to  complete  our  description  of  high  strain  rate 
deformation  is  one  which  allows  us  to  compute  the  temperature  change  during  the 
deformation.    In  the  absence  of  a  coupled  thermomechanical  finite  element  code  we 
assume  adiabatic  temperature  change  and  follow  the  empirical  assumption  that  90  -
 95% of the plastic work is dissipated as heat.  Hence, 
𝑇̇ =
0.9
𝜌𝐶v
(𝛔 ⋅ 𝐃p),
(22.41.10)
where 𝜌 is the density of the material and 𝐶v the specific heat. 
In terms of the input parameters the functions defined above become: 
𝑉(𝑇) = C1 ∙ exp(−C2/𝑇)
𝑌(𝑇) = C3 ∙ exp(C4/𝑇) 
𝑓 (𝑇) = C5 ∙ exp(−C6/𝑇) 
𝑟𝑑(𝑇) = C7 ∙ exp(−C8/𝑇) 
and the heat generation coefficient is 
ℎ(𝑇) = C9 ∙ exp(C10/𝑇) 
𝑟𝑠(𝑇) = C11 ∙ exp(−C12/𝑇) 
𝑅𝑑(𝑇) = C13 ∙ exp(−C14/𝑇) 
𝐻(𝑇) = C15 ∙ exp(C16/𝑇) 
𝑅𝑠(𝑇) = C17 ∙ exp(−C18/𝑇)
𝐻𝐶 =
0.9
𝜌𝐶𝑉
.
(22.41.11)
LS-DYNA Theory Manual 
Material Models 
22.42  Material Model 52:  Sandia’s Damage Model 
The evolution of the damage parameter, 𝜙, is defined by [Bammann, et.  al., 1990] 
𝜙̇ = 𝛽 [
(1 − 𝜙)𝑁 − (1 − 𝜙)]
∣Dp∣
,
in which 
where 𝑝 is the pressure and 𝜎̅̅̅̅̅ is the effective stress.
𝛽 = sin [
2(2𝑁 − 1)𝑝
(2𝑁 − 1)𝜎̅̅̅̅̅
], 
(22.42.1)
(22.42.2)
Material Models 
LS-DYNA Theory Manual 
22.43  Material Model 53:  Low Density Closed Cell 
Polyurethane Foam 
A rigid, low density, closed cell, polyurethane foam model developed at Sandia 
Laboratories [Neilsen  et al., 1987] has  been recently implemented for modeling impact 
limiters in automotive applications.  A number of such foams were tested at Sandia and 
reasonable fits to the experimental data were obtained.  
In some respects this model is similar to the crushable honeycomb model type 26 
in  that  the  components  of  the  stress  tensor  are  uncoupled  until  full  volumetric 
compaction is achieved.  However, unlike the honeycomb model this material possesses 
no directionality but includes the effects of confined air pressure in its overall response 
characteristics. 
where 𝜎𝑖𝑗
sk is the skeletal stress and 𝜎 air is the air pressure computed from the equation: 
𝜎𝑖𝑗 = 𝜎𝑖𝑗
sk − δ𝑖𝑗𝜎 air,
(22.43.1)
𝜎 air = −
𝑝0𝛾
1 + 𝛾 − 𝜙
,
(22.43.2)
where 𝑝0  is  the  initial  foam  pressure  usually  taken  as  the  atmospheric  pressure  and  𝛾 
defines the volumetric strain  
𝛾 = 𝑉 − 1 + 𝛾0,
(22.43.3)
where 𝑉 is the relative volume and 𝛾0  is the initial volumetric strain which is typically 
zero.  The yield condition is applied to the principal skeletal stresses which are updated 
independently of the air pressure.  We first obtain the skeletal stresses: 
 𝜎𝑖𝑗
sk = 𝜎𝑖𝑗 + 𝜎𝑖𝑗𝜎 air,
and compute the trial stress, 𝛔𝑖
skt 
skt = 𝜎𝑖𝑗
𝜎𝑖𝑗
sk + 𝐸𝜀̇𝑖𝑗Δ𝑡,
(22.43.4)
(22.43.5)
where  𝐸  is  Young’s  modulus.    Since  Poisson’s  ratio  is  zero,  the  update  of  each  stress 
component  is  uncoupled  and  2𝐺 = 𝐸  where  𝐺  is  the  shear  modulus.    The  yield 
condition  is  applied  to  the  principal  skeletal  stresses  such  that  if  the  magnitude  of  a 
principal trial stress component, 𝛔𝑖
skt, exceeds the yield stress, 𝜎y, then 
sk = min(𝜎y, ∣𝛔𝑖
𝛔𝑖
skt∣)
skt
.
skt∣
𝛔𝑖
∣𝛔𝑖
The yield stress is defined by 
𝜎y = 𝑎 + 𝑏(1 + 𝑐𝛾),
22-134 (Material Models) 
(22.43.6)
LS-DYNA Theory Manual 
Material Models 
where 𝑎, 𝑏, and 𝑐 are user defined input constants.  After scaling the principal stresses 
they are transformed back into the global system and the final stress state is computed 
sk − 𝛿𝑖𝑗𝜎 air.
𝜎𝑖𝑗 = 𝜎𝑖𝑗
(22.43.8)
Material Models 
LS-DYNA Theory Manual 
22.44  Material Models 54 and 55:  Enhanced Composite 
Damage Model 
These  models  are  very  close  in  their  formulations.    Material  54  uses  the  Chang 
matrix failure criterion (as Material 22), and material 55 uses the Tsay-Wu criterion for 
matrix failure. 
Arbitrary  orthothropic  materials,  e.g.,  unidirectional  layers  in  composite  shell 
structures  can  be  defined.    Optionally,  various  types  of  failure  can  be  specified 
following either the suggestions of [Chang and Chang, 1984] or [Tsai and Wu, 1981].  In 
addition special measures are taken for failure under compression.  See [Matzenmiller 
and Schweizerhof, 1990].  This model is only valid for thin shell elements. 
The Chang/Chang criteria is given as follows: for the tensile fiber mode, 
𝜎aa > 0    then    𝑒f
2 = (
𝜎aa
Xt
)
+ 𝛽 (
)
𝜎𝑎𝑏
𝑆𝑐
− 1 {≥ 0 failed
, 
< 0 elastic
for the compressive fiber mode, 
Ea = Eb = Gab = νba = νab = 0,
𝜎aa < 0    then    𝑒c
2 = (
𝜎aa
Xc
)
− 1 {≥ 0 failed
< 0 elastic
,
for the tensile matrix mode,  
Ea = νba = νab = 0,
𝜎bb > 0    then    𝑒m
2 = (
𝜎bb
Yt
)
+ (
𝜎ab
Sc
)
− 1 {≥ 0 failed
, 
< 0 elastic
and for the compressive matrix mode, 
Eb = νba = 0 → Gab = 0,
(22.44.1) 
(22.44.2)
(22.44.3) 
(22.44.4)
(22.44.5) 
(22.44.6)
𝜎bb < 0    then    𝑒d
2 = (
𝜎bb
2Sc
)
+
)
Yc
2Sc
⎢⎡(
⎣
− 1
⎥⎤ 𝜎bb
Yc
⎦
+ (
)
𝜎ab
Sc
− 1 {≥ 0 failed
< 0  elastic
, 
(22.44.7) 
Eb = νba = νab = 0 ⇒
Gab = 0
XC = 2Yc,
for 50% fiber volume
.
(22.44.8) 
In the Tsay/Wu criteria the tensile and compressive fiber modes are treated as in 
the Chang/Chang criteria.   The failure criterion for the tensile and compressive matrix 
mode is given as:
LS-DYNA Theory Manual 
Material Models 
2 =
𝑒md
𝜎bb
YcYt
+ (
𝜎ab
Sc
)
+
(Yc − Yt) 𝜎bb
YcYt
− 1 {≥ 0 failed
< 0 elastic
. 
(22.44.9)
For 𝛽 = 1  we  get  the  original  criterion  of  Hashin  [1980]  in  the  tensile  fiber  mode.    For 
𝛽 = 0,  we  get  the  maximum  stress  criterion  which  is  found  to  compare  better  to 
experiments. 
Failure can occur in any of four different ways: 
1. 
2. 
3. 
4. 
If  DFAILT  is  zero,  failure  occurs  if  the  Chang/Chang  failure  criterion  is 
satisfied in the tensile fiber mode. 
If DFAILT is greater than zero, failure occurs if the tensile fiber strain is greater 
than DFAILT or less than DFAILC. 
If  EFS  is  greater than  zero,  failure  occurs  if  the  effective  strain  is  greater  than 
EFS. 
If TFAIL is greater than zero, failure occurs according to the element time step 
as described in the definition of TFAIL above. 
When  failure  has  occurred  in  all  the  composite  layers  (through-thickness 
integration  points),  the  element  is  deleted.    Elements  which  share  nodes  with  the 
deleted element become “crashfront” elements and can have their strengths reduced by 
using the SOFT parameter with TFAIL greater than zero. 
Information about the status in each layer (integration point) and element can be 
plotted  using  additional  integration  point  variables.    The  number  of  additional 
integration  point  variables  for  shells  written to the  LS-DYNA  database  is  input  by  the 
*DATABASE_BINARY  definition  as  variable  NEIPS.    For  Models  54  and  55  these 
additional variables are tabulated below (i = shell integration point): 
History 
Variable 
Description 
Value 
1. 𝑒𝑓 (𝑖) 
2. 𝑒𝑐(𝑖) 
3. 𝑒𝑚(𝑖) 
4. 𝑒𝑑(𝑖) 
tensile fiber mode 
compressive fiber mode 
tensile matrix mode 
compressive 
mode 
matrix 
5. 𝑒𝑓𝑎𝑖l  max[𝑒𝑓 (𝑖𝑝)] 
6. 𝑑𝑎𝑚 
damage parameter 
1 – elastic 
0 – failed 
-1 - element intact 
10-8 - element in crashfront 
+1 - element failed 
LS-PREPOST 
History 
Variable 
1 
2 
3 
4 
5
Material Models 
LS-DYNA Theory Manual 
The  following  components,  defined  by  the  sum  of  failure  indicators  over  all 
through-thickness integration points, are stored as element component 7 instead of the 
effective plastic strain.: 
𝑛𝑖𝑝
Description 
𝑛𝑖𝑝
∑ 𝑒𝑓 (𝑖)
𝑖=1
𝑛𝑖𝑝
∑ 𝑒𝑐(𝑖)
𝑖=1
𝑛𝑖𝑝
∑ 𝑐𝑚(𝑖)
𝑖=1
𝑛𝑖𝑝
𝑛𝑖𝑝
Integration point 
1 
2
LS-DYNA Theory Manual 
Material Models 
22.45  Material Model 57:  Low Density Urethane Foam 
The urethane foam model is available to model highly compressible foams such 
as those used in seat cushions and as padding on the Side Impact Dummy (SID).  The 
compressive  behavior  is  illustrated  in  Figure  22.45.1  where  hysteresis  on  unloading  is 
shown.  This behavior under uniaxial loading is assumed not to significantly couple in 
the  transverse  directions.    In  tension  the  material  behaves  in  a  linear  fashion  until 
tearing  occurs.    Although  our  implementation  may  be  somewhat  unusual,  it  was  first 
motivated by Shkolnikov [1991] and a paper by Storakers [1986].  The recent additions 
necessary to model hysteretic unloading and rate effects are due to Chang, et al., [1994].  
These latter additions have greatly expanded the usefulness of this model. 
The  model  uses  tabulated  input  data  for  the  loading  curve  where  the  nominal 
stresses are defined as a function of the elongations, 𝜀𝑖, which are defined in terms of the 
principal stretches, 𝜆𝑖, as: 
𝜀𝑖 = 𝜆 𝑖 − 1.
(22.45.1)
The  stretch  ratios  are  found  by  solving  for  the  eigenvalues  of  the  left  stretch 
tensor,  𝑉𝑖𝑗,  which  is  obtained  via  a  polar  decomposition  of  the  deformation  gradient 
matrix, 𝐹𝑖𝑗: 
𝐹𝑖𝑗 = 𝑅𝑖𝑘𝑈𝑘𝑗 = 𝑉𝑖𝑘𝑅𝑘𝑗.
(22.45.2)
The  update  of  𝑉𝑖𝑗  follows  the  numerically  stable  approach  of  Taylor  and 
Flanagan [1989].  After solving for the principal stretches, the elongations are computed 
and,  if  the  elongations  are  compressive,  the  corresponding  values  of  the  nominal 
stresses, 𝜏𝑖 are interpolated.  If the elongations are tensile, the nominal stresses are given 
by 
Typical unloading
curves determined by
the hysteretic unloading
factor. With the shape
factor equal to unity.
Typical unloading for
a large shape factor, e.g. 
5.0-8.0, and a small 
hystereticfactor, e.g., 0.010.
Unloading
curves
Strain
Strain
Figure 22.45.1.  Behavior of the low-density urethane foam model.
Material Models 
LS-DYNA Theory Manual 
𝜏𝑖 = 𝐸𝜀𝑖.
The Cauchy stresses in the principal system become 
𝜎𝑖 =
𝜏𝑖
𝜆𝑗𝜆𝑘
.
(22.45.3)
(22.45.4)
The  stresses  are  then  transformed  back  into  the  global  system  for  the  nodal  force 
calculations. 
When hysteretic unloading is used, the reloading will follow the unloading curve 
if the decay constant, 𝛽, is set to zero.  If 𝛽 is nonzero the decay to the original loading 
curve is governed by the expression: 
1 − 𝑒−𝛽𝑡.
(22.45.5)
The  bulk  viscosity,  which  generates  a  rate  dependent  pressure,  may  cause  an 
unexpected volumetric response and, consequently, it is optional with this model.   
Rate  effects  are  accounted  for  through  linear  viscoelasticity  by  a  convolution 
integral of the form 
r = ∫ 𝑔𝑖𝑗𝑘𝑙
𝜎𝑖𝑗
where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) is the relaxation function.  The stress tensor, 𝜎𝑖𝑗
determined  from  the  foam,  𝜎𝑖𝑗
summation of the two contributions: 
(𝑡 − 𝜏)
r , augments the stresses 
f ;  consequently,  the  final  stress,  𝜎𝑖𝑗,  is  taken  as  the 
(22.45.6)
𝑑𝜏,
∂𝜀𝑘𝑙
∂𝜏
𝜎𝑖𝑗 = 𝜎𝑖𝑗
r .
f + 𝜎𝑖𝑗
(22.45.7)
Since  we  wish  to  include  only  simple  rate  effects,  the  relaxation  function  is 
represented by one term from the Prony series: 
given by, 
𝑔(𝑡) = 𝛼0 + ∑ α𝑚
𝑚=1
𝑒−𝛽𝑡,
𝑔(𝑡) = 𝐸d𝑒−𝛽1𝑡.
(22.45.8)
(22.45.9)
This model is effectively a Maxwell fluid which consists of a damper and spring 
in  series.    We  characterize  this  in  the  input  by  a  Young's  modulus,  𝐸d,  and  decay 
constant,  𝛽1.    The  formulation  is  performed  in  the  local  system  of  principal  stretches 
where only the principal values of stress are computed and triaxial coupling is avoided.  
Consequently,  the  one-dimensional  nature  of  this  foam  material  is  unaffected  by  this 
addition  of  rate  effects.    The  addition  of  rate  effects  necessitates  twelve  additional
LS-DYNA Theory Manual 
Material Models 
history  variables  per  integration  point.    The  cost  and  memory  overhead  of  this  model 
comes primarily from the need to “remember” the local system of principal stretches. 
Viscous  damping  is  implemented  by  incrementation  of  the  principal  stress 
components.  Firstly, we let 
𝑎 =
𝑐𝜌𝜇𝐿𝑒
1 + 𝛾
,
(22.45.10)
where 𝑐,  𝜌,  𝜇,  𝐿𝑒  and  𝛾  respectively  denote  the  material  sound  speed,  density,  viscous 
  The 
coefficient,  element  characteristic 
incremental stress components due to viscous damping are then given by  
length  and  element  volumetric  strain. 
Δ𝜎𝑖 = 𝑎 (
𝜀̇𝑖 − 𝜀̇𝑚
1 + 𝜈
+
𝜀̇𝑚
1 − 2𝜈
) 𝑖 = 1,2,3 
and 
Δ𝜎𝑖 =
𝑎𝜀̇𝑖
2(1 + 𝜈)
𝑖 = 4,5,6, 
where 𝜀̇𝑖 are the strain rates and 𝜀̇𝑚 = ∑ 𝜀̇𝑖
𝑖=1
3⁄ .
(22.45.11)
(22.45.12)
Material Models 
LS-DYNA Theory Manual 
22.46  Material Model 58:  Laminated Composite Fabric 
Parameters  to  control  failure  of  an  element  layer  are:  ERODS,  the  maximum 
effective  strain,  i.e.,  maximum  1 = 100%  straining.    The  layer  in  the  element  is 
completely  removed  after  the  maximum  effective  strain  (compression/tension 
including shear) is reached.   
The stress limits are factors used to limit the stress in the softening part to a given 
value,  
𝜎min = SLIMxx ⋅ strength,
(22.46.1)
thus,  the  damage  value  is  slightly  modified  such  that    elastoplastic  like  behavior  is 
achieved with the threshold stress.  As a factor for SLIMxx a number between 0.0 and 
1.0 is possible.  With a factor of 1.0, the stress remains at a maximum value identical to 
the strength, which is similar to ideal elastoplastic behavior.  For tensile failure a small 
value  for  SLIMTx  is  often  reasonable;  however,  for  compression  SLIMCx = 1.0  is 
preferred.    This  is  also  valid  for  the  corresponding  shear  value.    If  SLIMxx  is  smaller 
than  1.0  then  localization  can  be  observed  depending  on  the  total behavior  of  the  lay-
up.    If  the  user  is  intentionally  using  SLIMxx < 1.0,  it  is  generally  recommended  to 
avoid  a  drop  to  zero  and  set  the  value  to  something  in  between  0.05  and  0.10.  Then 
elastoplastic  behavior  is  achieved  in  the  limit  which  often  leads  to  less  numerical 
problems.  Defaults for SLIMXX = 1.0E-8. 
The  crashfront-algorithm  is  started  if  and  only  if  a  value  for  TSIZE  (time  step 
size, with element elimination after the actual time step becomes smaller than TSIZE) is 
input . 
The  damage  parameters  can  be  written  to  the  postprocessing  database  for  each 
integration point as the first three additional element variables and can be visualized. 
Material  models  with  FS = 1  or  FS = −1  are  favorable  for  complete  laminates 
and fabrics, as all directions are treated in a similar fashion. 
For  material  model  FS = 1  an  interaction  between  normal  stresses  and  shear 
stresses  is  assumed  for  the  evolution  of  damage  in  the  a-  and  b-  directions.    For  the 
shear damage is always the maximum value of the damage from the criterion in a- or b- 
direction is taken. 
For  material  model  FS = −1  it  is  assumed  that  the  damage  evolution  is 
independent  of  any  of  the  other  stresses.    A  coupling  is  present  only  via  the  elastic 
material parameters and the complete structure.
LS-DYNA Theory Manual 
Material Models 
SC
TAU1
SLIMS*SC
GAMMA1
GMS
Figure 22.46.1.  Stress-strain diagram for shear. 
In tensile and compression directions and in a- as well as in b- direction, different 
failure surfaces can be assumed.  The damage values, however, increase only when the 
loading direction changes. 
Special control of shear behavior of fabrics 
For  fabric  materials  a  nonlinear  stress  strain  curve  for  the  shear  part  of  failure 
surface FS = −1 can be assumed as given below.  This is not possible for other values of 
FS. 
The curve, shown in Figure 22.46.1, is defined by three points: 
•  the origin (0,0) is assumed, 
•  the  limit  of  the  first  slightly  nonlinear  part  (must  be  input),  stress  (TAU1)  and 
strain (GAMMA1), see below. 
•  the shear strength at failure and shear strain at failure. 
In addition a stress limiter can be used to keep the stress constant via the SLIMS 
parameter.  This value must be less than or equal to 1.0 and positive, which leads to an 
elastoplastic behavior for the shear part.  The default is 1.0E-08, assuming almost brittle 
failure once the strength limit SC is reached.
Material Models 
LS-DYNA Theory Manual 
22.47  Material Model 60:  Elastic With Viscosity 
This  material  model  was  developed  to  simulate  the  forming  of  glass  products 
(e.g., car windshields) at high temperatures.  Deformation is by viscous flow but elastic 
deformations  can  also  be  large.    The  material  model,  in  which  the  viscosity  may  vary 
with temperature, is suitable for treating a wide range of viscous flow problems and is 
implemented for brick and shell elements. 
Volumetric  behavior  is  treated  as  linear  elastic.    The  deviatoric  strain  rate  is 
considered to be the sum of elastic and viscous strain rates: 
𝛆̇′total = 𝛆̇′elastic + 𝛆̇′ viscous =
𝛔̇′
2𝐺
+
𝛔̇′
2𝜈
,
(22.47.1)
where 𝐺 is the elastic shear modulus, 𝜈 is the viscosity coefficient.  The stress increment 
over one time step 𝑑𝑡 is 
𝑑𝛔′ = 2𝐺𝛆̇′total𝑑𝑡 −
𝑑𝑡𝛔′.
(22.47.2)
The  stress  before  the  update  is  used  for  𝛔′.    For  shell  elements,  the  through-
thickness strain rate is calculated as follows 
𝑑𝜎33 = 0 = 𝐾(𝜀̇11 + 𝜀̇22 + 𝜀̇33)𝑑𝑡 + 2𝐺𝜀̇′33 𝑑𝑡 −
𝑑𝑡σ′
33,
(22.47.3)
where the subscript 𝑖𝑗 = 33 denotes the through-thickness direction and 𝐾 is the elastic 
bulk modulus.  This leads to: 
𝜀̇33 = −a(𝜀̇11 + 𝜀̇22) + 𝑏𝑝,
𝑎 =
𝐾 − 2
𝐾 + 4
, 
𝑏 =
𝐺𝑑𝑡
𝜐(𝐾 + 4
,
𝐺)
(22.47.4) 
(22.47.5) 
(22.47.6) 
in which 𝑝 is the pressure defined as the negative of the hydrostatic stress.
LS-DYNA Theory Manual 
Material Models 
22.48  Material Model 61:  Maxwell/Kelvin Viscoelastic with 
Maximum Strain 
The shear relaxation behavior is described for the Maxwell model by: 
𝐺(𝑡) = G∞ + (G0 − G∞)𝑒−𝛽𝑡.
A Jaumann rate formulation is used 
∇
𝑠′𝑖𝑗
= 2 ∫ 𝐺(𝑡 − 𝜏)𝜀′̇
𝑖𝑗(𝜏)𝑑𝑡
,
(22.48.1)
(22.48.2)
∇
where  the  prime  denotes  the  deviatoric  part  of  the  stress  rate,  𝑠′𝑖𝑗
deviatoric strain rate. 
,  and  𝜀̇′𝑖𝑗  is  the 
For the Kelvin model the stress evolution equation is defined as: 
𝑠 ̇𝑖𝑗 +
𝑠𝑖𝑗 = (1 + 𝛿𝑖𝑗)G0𝜀′̇
𝑖𝑗 + (1 + 𝛿𝑖𝑗)
G∞
𝜀′𝑖𝑗,
(22.48.3)
where 𝛿𝑖𝑗 is the Kronecker delta, G0 is the instantaneous shear modulus, G∞is the long 
term shear modulus, and τ is the decay constant.   
The pressure is determined from the bulk modulus and the volumetric strain: 
where 
𝑝 = −𝐾𝜀v,
𝜀v = ln (
𝑉0
),
(22.48.4)
(22.48.5)
defines the logarithmic volumetric strain from the relative volume. 
Bandak’s  [1991]  calculation  of  the  total  strain  tensor,  𝜀𝑖𝑗,  for  output  uses  an 
incremental update based on Jaumann rate: 
𝑛+1 = 𝜀𝑖𝑗
𝜀𝑖𝑗
𝑛 + 𝑟𝑖𝑗
𝑛 + 𝜀𝑖𝑗
𝛻𝑛+1
2⁄
𝛥𝑡𝑛+1
2⁄ ,
where 
𝑛+1
2⁄
𝛥𝜀𝑖𝑗
𝑛+1
2⁄
𝛥𝑡𝑛+1
2⁄ ,
= 𝜀̇𝑖𝑗
and 𝑟𝑖𝑗
𝑛 gives the rotation of the stain tensor at time 𝑡𝑛 to the configuration at 𝑡𝑛+1 
𝑛 = (𝜀𝑖𝑝
𝑟𝑖𝑗
𝑛 𝜔𝑝𝑗
𝑛+1
2⁄
+ 𝜀𝑗𝑝
𝑛 𝜔𝑝𝑖
𝑛+1
2⁄
) 𝛥𝑡𝑛+1
2⁄ .
(22.48.6)
(22.48.7)
(22.48.8)
Material Models 
LS-DYNA Theory Manual 
22.49  Material Model 62:  Viscous Foam 
This model was written to represent the energy absorbing foam found on certain 
crash dummies, i.e., the ‘Confor Foam’ covering the ribs of the Eurosid dummy. 
The  model  consists  of  a  nonlinear  elastic  stiffness  in  parallel  with  a  viscous 
damper.    A  schematic  is  shown  in  Figure  22.49.1.    The  elastic  stiffness  is  intended  to 
limit  total  crush  while  the  viscous  damper  absorbs  energy.    The  stiffness  𝐸2  prevents 
timestep problems.   
Both 𝐸1 and 𝑉2 are nonlinear with crush as follows: 
𝑡 = 𝐸1(𝑉−n1),
𝐸1
𝑡 = 𝑉2(abs(1 − 𝑉))
𝑉2
n2,
(22.49.1)
where  𝑉  is  the  relative  volume  defined  by  the  ratio  of  the  current  to  initial  volume.  
Typical values are (units of N, mm, s) 
(22.49.2)
𝐸1 = 0.0036,
𝑛1 = 4.0, 
𝑉2 = 0.0015, 
𝐸2 = 100.0, 
𝑛2 = 0.2, 
𝜈 = 0.05.
E1
V1
E2
Figure 22.49.1.  Schematic of Material Model 62.
LS-DYNA Theory Manual 
Material Models 
22.50  Material Model 63:  Crushable Foam 
The  intent  of  this  model  is  to  model  crushable  foams  in  side  impact  and  other 
applications where cyclic behavior is unimportant. 
This isotropic foam model crushes one-dimensionally with a Poisson’s ratio that 
is essentially zero.  The stress versus strain behavior is depicted in Figure 22.50.1 where 
an example of unloading from point a to the tension cutoff stress at b then unloading to 
point c and finally reloading to point d is shown.  At point d the reloading will continue 
along the loading curve.  It is important to use nonzero values for the tension cutoff to 
prevent the disintegration of the material under small tensile loads.  For high values of 
tension  cutoff  the  behavior of  the  material will  be  similar  in  tension  and  compression.  
Viscous  damping in the model follows an implementation identical to that of material 
type 57. 
In the implementation we assume that Young’s modulus is constant and update 
the stress assuming elastic behavior. 
trial = 𝜎𝑖𝑗
𝜎𝑖𝑗
𝑛 + 𝐸𝜀̇𝑖𝑗
𝑛+1
2⁄
Δ𝑡𝑛+1
2⁄ .
(22.50.1)
The magnitudes of the principal values, 𝜎𝑖
stress, 𝜎y, is exceeded and if so they are scaled back to the yield surface: 
trial, 𝑖 = 1,3  are then checked to see if the yield 
if  𝜎y < ∣𝜎𝑖
trial∣
then 𝜎𝑖
𝑛+1 = 𝜎y
trial
.
trial∣
𝜎𝑖
∣σ𝑖
(22.50.2)
After  the  principal  values  are  scaled,  the  stress  tensor  is  transformed  back  into 
ij
Volumetric strain - In V
Figure  22.50.1.    Yield  stress  versus  volumetric  strain  curve  for  the  crushable
foam.
Material Models 
LS-DYNA Theory Manual 
the global system.  As seen in Figure 22.50.1, the yield stress is a function of the natural 
logarithm of the relative volume, 𝑉, i.e., the volumetric strain.
LS-DYNA Theory Manual 
Material Models 
22.51  Material Model 64:  Strain Rate Sensitive Power-Law 
Plasticity 
This material model follows a constitutive relationship of the form: 
𝜎 = 𝑘𝜀𝑚𝜀̇𝑛
(22.51.1)
where 𝜎 is the yield stress, 𝜀 is the effective plastic strain, 𝜀̇ is the effective plastic strain 
rate,  and  the  constants  𝑘,  𝑚,  and  𝑛  can  be  expressed  as  functions  of  effective  plastic 
strain  or  can  be  constant  with  respect  to  the  plastic  strain.    The  case  of  no  strain 
hardening can be obtained by setting the exponent of the plastic strain equal to a very 
small positive value, i.e., 0.0001. 
This  model  can  be  combined  with  the  superplastic  forming  input  to  control  the 
magnitude  of  the  pressure  in  the  pressure  boundary  conditions  in  order  to  limit  the 
effective  plastic  strain  rate  so  that  it  does  not  exceed  a  maximum  value  at  any 
integration point within the model.   
A  fully  viscoplastic  formulation  is  optional.    An  additional  cost  is  incurred  but 
the improvement in results can be dramatic.
Material Models 
LS-DYNA Theory Manual 
22.52  Material Model 65:  Modified Zerilli/Armstrong 
The  Armstrong-Zerilli  Material  Model  expresses  the  flow  stress  as  follows.    For 
fcc metals, 
𝜎 = C1 + {C2(𝜀p)
2⁄ [𝑒(−C3+C4ln(𝜀̇∗))𝑇] + C5} (
𝜇(𝑇)
𝜇(293)
),
(22.52.1)
𝜀p =  effective plastic strain 
𝜀̇∗ =
𝜀̇
𝜀̇0
 effective plastic strain rate  
where  𝜀̇0 = 1,1𝑒 − 3,1𝑒 − 6  for  time  units  of  seconds,  milliseconds,  and  microseconds, 
respectively. 
For bcc metals, 
𝜎 = C1 + C2𝑒(−C3+C4ln(𝜀̇∗))𝑇 + [C5(𝜀p)𝑛 + C6] (
𝜇(𝑇)
𝜇(293)
), 
(22.52.2)
where 
(
𝜇(𝑇)
𝜇(293)
) = B1 + B2𝑇 + B3𝑇2.
(22.52.3)
The  relationship  between  heat  capacity  (specific  heat)  and  temperature  may  be 
characterized by a cubic polynomial equation as follows: 
Cp = G1 + G2𝑇 + G3𝑇2 + G4𝑇3.
(22.52.4)
A  fully  viscoplastic  formulation  is  optional.    An  additional  cost  is  incurred  but 
the improvement in results can be dramatic.
LS-DYNA Theory Manual 
Material Models 
22.53  Material Model 66:  Linear Stiffness/Linear Viscous 3D 
Discrete Beam 
The formulation of the discrete beam (Type 6) assumes that the beam is of zero 
length and requires no orientation node.  A small distance between the nodes joined by 
the  beam  is  permitted.    The  local  coordinate  system  which  determines  (𝑟, 𝑠, 𝑡)  is  given 
by the coordinate ID in the cross sectional input where the global system is the default.  
The  local  coordinate  system  axes  rotate  with  the  average  of  the  rotations  of  the  two 
nodes that define the beam. 
For  null  stiffness  coefficients,  no  forces  corresponding  to  these  null  values  will 
develop.  The viscous damping coefficients are optional.
Material Models 
LS-DYNA Theory Manual 
22.54  Material Model 67:  Nonlinear Stiffness/Viscous 3D 
Discrete Beam 
The formulation of the discrete beam (Type 6) assumes that the beam is of zero 
length and requires no orientation node.  A small distance between the nodes joined by 
the  beam  is  permitted.    The  local  coordinate  system  which  determines  (𝑟, 𝑠, 𝑡)  is  given 
by the coordinate ID in the cross sectional input where the global system is the default.  
The  local  coordinate  system  axes  rotate  with  the  average  of  the  rotations  of  the  two 
nodes that define the beam. 
For null load curve ID’s, no forces are computed.   The force resultants are found 
from  load  curves    that  are  defined  in  terms  of  the  force  resultant 
versus the relative displacement in the local coordinate system for the discrete beam.
(b.)
(a.)
DISPLACEMENT
Figure 22.54.1.  The resultant forces and moments are determined by a table
lookup.    If  the  origin  of  the  load  curve  is  at  [0,0]  as  in  (b.)  and  tension  and
compression responses are symmetric. 
|DISPLACEMENT|
LS-DYNA Theory Manual 
Material Models 
22.55  Material Model 68:  Nonlinear Plastic/Linear Viscous 
3D Discrete Beam 
The formulation of the discrete beam (Type 6) assumes that the beam is of zero 
length and requires no orientation node.  A small distance between the nodes joined by 
the  beam  is  permitted.    The  local  coordinate  system  which  determines  (𝑟, 𝑠, 𝑡)  is  given 
by the coordinate ID in the cross sectional input where the global system is the default.  
The  local  coordinate  system  axes  rotate  with  the  average  of  the  rotations  of  the  two 
nodes that define the beam.  Each force resultant in the local system can have a limiting 
value  defined  as  a  function  of  plastic  displacement  by  using  a  load  curve  .  For the degrees of freedom where elastic behavior is desired, the load curve ID 
is simply set to zero. 
Catastrophic failure, based on force resultants, occurs if the following inequality 
is satisfied:   
(
𝐹r
fail
𝐹r
)
+ (
𝐹s
fail
𝐹s
)
+ (
𝐹t
fail
𝐹t
)
+ (
𝑀r
fail
𝑀r
)
+ (
𝑀s
fail
𝑀s
)
+ (
𝑀t
fail
𝑀t
)
− 1. ≥ 0. 
(22.55.1)
Likewise, catastrophic failure based on displacement resultants occurs if: 
(
𝑢r
fail
𝑢r
)
+ (
𝑢s
fail
𝑢s
)
+ (
𝑢t
fail
𝑢t
)
+ (
𝜃r
fail
𝜃r
)
+ (
𝜃s
fail
𝜃s
)
+ (
𝜃t
fail
𝜃t
)
− 1. ≥ 0. 
(22.55.2)
After failure, the discrete element is deleted.  If failure is included, either one or 
both of the criteria may be used.
PLASTIC DISPLACEMENT
Figure  22.55.1.    The  resultant  forces  and  moments  are  limited  by  the  yield
definition.  The initial yield point corresponds to a plastic displacement of zero.
Material Models 
LS-DYNA Theory Manual 
22.56  Material Model 69:  Side Impact Dummy Damper (SID 
Damper) 
The  side  impact  dummy  uses  a  damper  that  is  not  adequately  treated  by 
nonlinear  force  versus  relative  velocity  curves,  since  the  force  characteristics  are  also 
dependent  on  the  displacement  of  the  piston.    As  the  damper  moves,  the  fluid  flows 
through the open orifices to provide the necessary damping resistance.  While moving 
as  shown  in  Figure  22.56.1,  the  piston  gradually  blocks  off  and  effectively  closes  the 
orifices.    The  number  of  orifices  and  the  size  of  their  openings  control  the  damper 
resistance and performance.  The damping force is computed from the equation: 
𝐹 = 𝑆𝐹
{⎧
⎩{⎨
𝐾𝐴p𝑉p
{⎧𝐶1
⎩{⎨
𝐴0
𝑡 + 𝐶2∣𝐕p∣𝜌fluid
𝐴p
𝐶𝐴0
𝑡 )
⎡(
⎢
⎣
− 1
}⎫
⎭}⎬
⎤
⎥
⎦
}⎫
− 𝑓 (𝑠 + 𝑠0) + 𝑉p𝑔(𝑠 + 𝑠0)
⎭}⎬
,  (22.56.1)
where 𝐾 is a user defined constant or a tabulated function of the absolute value of the 
relative velocity, 𝐕p is the piston's relative velocity, 𝐶 is the discharge coefficient, 𝐴p is 
𝑡  is the total open areas of orifices at time 𝑡, 𝜌fluid is the fluid density, 
the piston area, 𝐴0
𝐶1 is the coefficient for the linear term, and 𝐶2 is the coefficient for the quadratic term. 
d4
d3
d2
d1
Piston
Vp
ith Piston Orifice
Orifice Opening Controller
  Figure 22.56.1.  Mathematical model for the Side Impact Dummy damper. 
2Ri - h
LS-DYNA Theory Manual 
Material Models 
Last orifice
closes.
Force increases as orifice
is gradually covered.
DISPLACEMENT
Figure 22.56.2.  Force versus displacement as orifices are covered at a constant 
relative velocity.  Only the linear velocity term is active. 
In  the  implementation,  the  orifices  are  assumed  to  be  circular  with  partial 
covering  by  the  orifice  controller.    As  the  piston  closes,  the  closure  of  the  orifice  is 
gradual.  This gradual closure is taken into account to insure a smooth response.  If the 
piston  stroke  is  exceeded,  the  stiffness  value,  𝑘,  limits  further  movement,  i.e.,  if  the 
damper  bottoms  out  in  tension  or  compression,  the  damper  forces  are  calculated  by 
replacing the damper by a bottoming out spring and damper, k and c, respectively.  The 
piston  stroke  must  exceed  the  initial  length  of  the  beam  element.    The  time  step 
calculation is based in part on the stiffness value of the bottoming out spring.  A typical 
force versus displacement curve at constant relative velocity is shown in Figure 22.56.2.  
The  factor, SF,  which  scales  the  force  defaults  to  1.0  and  is  analogous  to  the  adjusting 
ring on the damper.
Material Models 
LS-DYNA Theory Manual 
22.57  Material Model 70:  Hydraulic/Gas Damper 
This  special  purpose  element  represents  a  combined  hydraulic  and  gas-filled 
damper which has a variable orifice coefficient.  A schematic of the damper is shown in 
Figure  22.57.1.    Dampers  of  this  type  are  sometimes  used  on  buffers  at  the  end  of 
railroad tracks and as aircraft undercarriage shock absorbers.  This material can be used 
only as a discrete beam element. 
As  the  damper  is  compressed  two  actions  contribute to  the  force that  develops.  
First, the gas is adiabatically compressed into a smaller volume.  Secondly, oil is forced 
through  an orifice.   A profiled  pin  may occupy  some  of  the  cross-sectional  area  of the 
orifice;  thus,  the  orifice  area  available  for  the  oil  varies  with  the  stroke.    The  force  is 
assumed  proportional  to  the  square  of  the  velocity  and  inversely  proportional  to  the 
available area.  The equation for this element is: 
𝐹 = SCLF ⋅ {𝐾h (
𝑎0
)
+ [𝑃0 (
𝐶0
𝐶0 − 𝑆
)
− 𝑃a] ⋅ 𝐴p},
(22.57.1)
where 𝑆 is the element deflection and 𝑉 is the relative velocity across the element.
Orifice
Oil
Profiled Pin
Gas
Figure 22.57.1.  Schematic of Hydraulic/Gas damper.
LS-DYNA Theory Manual 
Material Models 
22.58  Material Model 71:  Cable 
This  material  can  be  used  only  as  a  discrete  beam  element.    The  force,  𝐹, 
generated by the cable is nonzero only if the cable is in tension.  The force is given by: 
𝐹 = 𝐾 ⋅ max(Δ𝐿, 0. ),
(22.58.1)
where Δ𝐿 is the change in length 
Δ𝐿 = current  length − (initial  length-offset),
(22.58.2)
and the stiffness is defined as: 
𝐾 =
𝐸 ⋅ area
(initial  length-  offset)
.
(22.58.3)
The area and offset are defined on either the cross section or element cards in the 
LS-DYNA input.  For a slack cable the offset should be input as a negative length.  For 
an  initial  tensile  force  the  offset  should  be  positive.    If  a  load  curve  is  specified,  the 
Young’s modulus will be ignored and the load curve will be used instead.  The points 
on  the  load  curve  are  defined  as  engineering  stress  versus  engineering  strain,  i.e.,  the 
change in length over the initial length.  The unloading behavior follows the loading.
Material Models 
LS-DYNA Theory Manual 
22.59  Material Model 73:  Low Density Viscoelastic Foam  
This  viscoelastic  foam  model  is  available  to  model  highly  compressible  viscous 
foams.    The  hyperelastic  formulation  of  this  model  follows  that  of  material  57.    Rate 
effects are accounted for through linear viscoelasticity by a convolution integral of the 
form 
r = ∫ 𝑔𝑖𝑗𝑘𝑙
𝜎𝑖𝑗
where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) is the relaxation function.  The stress tensor, 𝜎𝑖𝑗
determined  from  the  foam,  𝜎𝑖𝑗
summation of the two contributions: 
(𝑡 − 𝜏)
r , augments the stresses 
f ;  consequently,  the  final  stress,  𝜎𝑖𝑗,  is  taken  as  the 
(22.59.1)
𝑑𝜏,
𝜕𝜀𝑘𝑙
𝜕𝜏
𝜎𝑖𝑗 = 𝜎𝑖𝑗
r .
f + 𝜎𝑖𝑗
(22.59.2)
Since  we  wish  to  include  only  simple  rate  effects,  the  relaxation  function  is 
represented by up to six terms of the Prony series: 
𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚
𝑚=1
𝑒−𝛽𝑡.
(22.59.3)
This  model  is  effectively  a  Maxwell  fluid  which  consists  of  a  dampers  and 
springs in series.  The formulation is performed in the local system of principal stretches 
where only the principal values of stress are computed and triaxial coupling is avoided.  
Consequently,  the  one-dimensional  nature  of  this  foam  material  is  unaffected  by  this 
addition  of  rate  effects.    The  addition  of  rate  effects  necessitates  42  additional  history 
variables  per  integration  point.    The  cost  and  memory  overhead  of  this  model  comes 
primarily from the need to “remember” the local system of principal stretches and the 
evaluation of the viscous stress components.  Viscous damping in the model follows an 
implementation identical to that of material type 57.
LS-DYNA Theory Manual 
Material Models 
22.60  Material Model 74:  Elastic Spring for the Discrete 
Beam 
This  model  permits  elastic  springs  with  damping  to  be  combined  and 
represented  with  a  discrete  beam  element  type  6.    Linear  stiffness  and  damping 
coefficients  can  be  defined,  and,  for  nonlinear  behavior,  a  force  versus  deflection  and 
force versus rate curves can be used.  Displacement based failure and an initial force are 
optional.  
If the linear spring stiffness is used, the force, F, is given by: 
where K is the stiffness constant, and D is the viscous damping coefficient.   
𝐹 = 𝐹0 + 𝐾Δ𝐿 + 𝐷Δ𝐿̇,
(22.60.1)
If  the  load  curve  ID  for 𝑓 (Δ𝐿)  is  specified,  nonlinear  behavior  is  activated.    For 
this case the force is given by: 
𝐹 = 𝐹0 + 𝐾 𝑓 (Δ𝐿) [1 + C1 ⋅ Δ𝐿̇ + C2 ⋅ sgn(Δ𝐿̇)ln (max {1. ,
∣Δ𝐿̇∣
DLE
})]
(22.60.2)
            +𝐷Δ𝐿̇ + 𝑔(Δ𝐿)ℎ(Δ𝐿̇),
where  C1  and  C2  are  damping  coefficients  for  nonlinear  behavior,  DLE  is  a  factor  to 
scale  time  units,  and  𝑔(Δ𝐿)  is  an  optional  load  curve  defining  a  scale  factor  versus 
deflection for load curve ID, ℎ(𝑑Δ𝐿/𝑑𝑡). 
In these equations, Δ𝐿 is the change in length  
Δ𝐿 = current  length-initial  length.
(22.60.3)
Failure can occur in either compression or tension based on displacement values 
of CDF and TDF, respectively.  After failure no forces are carried.  Compressive failure 
does not apply if the spring is initially zero length. 
The  cross  sectional  area  is  defined  on  the  section  card  for  the  discrete  beam 
elements,  in  *SECTION_BEAM.    The  square  root  of  this  area  is  used  as  the  contact 
thickness offset if these elements are included in the contact treatment.
Material Models 
LS-DYNA Theory Manual 
22.61  Material Model 75:  Bilkhu/Dubois Foam Model  
This  model  uses  uniaxial  and  triaxial  test  data  to  provide  a  more  realistic 
treatment of crushable foam.  The Poisson’s ratio is set to zero for the elastic response.  
The volumetric strain is defined in terms of the relative volume, 𝑉, as: 
𝛾 = −ln(𝑉).
(22.61.1)
In  defining  the  curves,  the  stress  and  strain  pairs  should  be  positive  values 
starting with a volumetric strain value of zero. 
Viscous  damping  in  the  model  follows  an  implementation  identical  to  that  of 
material type 57.
Uniaxial Yield Stress
Pressure Yield
Figure 22.61.1.  Behavior of crushable foam.  Unloading is elastic. 
Volumetric Strain
LS-DYNA Theory Manual 
Material Models 
22.62  Material Model 76:  General Viscoelastic  
22.62.1  Introduction 
Material type 76 in LS-DYNA is a general viscoelastic Maxwell model having up to 18 
terms  in  the  prony  series  expansion  and  is  useful  for  modeling  dense  continuum 
rubbers and solid explosives.  It is characterized in the input by bulk and shear modulii, 
𝑔 .  Either  the  coefficients  of  the 
𝐾𝑚  and  𝐺𝑚,  and  associated  decay  constants,  𝛽𝑚
prony  series  expansion  can  be  used  directly,  or  a  relaxation  curve  may  be  specified  to 
define the viscoelastic deviatoric and bulk behavior. 
𝑘   and  𝛽𝑚
22.62.2  Constitutive Model 
The model is a hypoelastic version of the model given by Christensen and can be stated 
as 
𝝈∇ = ∑(𝐾𝑚𝑡𝑚
∇ )
∇ 𝒊 + 2𝐺𝑚𝒔𝑚
,
(22.62.1)
where 𝑡𝑚 and 𝒔𝑚 are (strain) quantities governed by the following evolution in time 
∇ = 𝑫dev − 𝛽𝑚
𝒔𝑚
𝑔 𝒔𝑚
(22.62.2)
and 
𝑘 𝑡𝑚
∇ = 𝐷vol − 𝛽𝑚
𝑡𝑚
(22.62.3)
𝑔   are  the 
Here  𝐾𝑚  and  𝐺𝑚  are  bulk  and  shear  moduli,  respectively,  𝛽𝑚
corresponding decay coefficients, 𝐷vol and 𝑫dev are the volumetric and deviatoric strain 
rates,  𝒊  is  the  2nd  order  identity  tensor  and  ∇  denotes  the  Jaumann  objective  rate.    It 
should immediately be noted that for all decay coefficients equal to 0 (zero), the model 
is reduced to a time independent elastic model, 
𝑘   and  𝛽𝑚
𝝈 ∇ = 𝐾𝐷vol𝒊 + 2𝐺𝑫dev 
with  bulk  and  shear  modulus  given  by  𝐾 = ∑ 𝐾𝑚𝑚
displacement theory, the stress can be integrated to be given by 
  and  𝐺 = ∑ 𝐺𝑚𝑚
(22.62.4) 
.  For  small 
𝝈(𝑡) = ∑ (𝐾𝑚 ∫ 𝑒−𝛽𝑚
𝑘 (𝑡−𝜏)𝐷vol(𝜏)
𝑑𝜏𝒊 + 2𝐺𝑚 ∫ 𝑒−𝛽𝑚
𝑔 (𝑡−𝜏)𝑫dev(𝜏)
𝑑𝜏)
(22.62.5) 
For  shell  elements,  the  same  theory  applies  except  that  the  objective  rate  ∇  is  the 
corotational time derivative instead of the Jaumann rate. 
22.62.3  Tangent Modulus 
For the implicit tangent modulus, we note that the internal force contribution depends 
on the displacement and time, which we  denote 𝒇int = 𝒇int(𝒖, 𝑡). The time derivative of 
this  vector  is  the  sum  of  a  material  and  a  geometric  contribution.    The  material 
contribution is given by
Material Models 
LS-DYNA Theory Manual 
Stress relaxation curve
10n
10n+1
10n+2
time
Optional ramp time for loading
load  curve  should  be  equally  spaced  on  the 
Figure 22.62.1.  Relaxation curve.  This curve defines stress versus time where
time  is  defined  on  a  logarithmic  scale.    For  best  results,  the  points  defined  in
the 
logarithmic  scale.
Furthermore,  the  load  curve  should  be  smooth  and  defined  in  the  positive 
quadrant.  If nonphysical values are determined by least squares fit, LS-DYNA 
will terminate with an error message after the initialization phase is completed.
If  the  ramp  time  for  loading  is  included,  then  the  relaxation  which  occurs 
during the loading phase is taken into account.  This effect may or may not be
important. 
𝒇 ̇
mat = ∫ 𝑩𝑇 𝝈 ∇𝑇𝑑Ω 
int
(22.62.6) 
where  𝑩  is  the  strain  displacement  matrix,  the  integration  is  over  the  current 
configuration  Ω  and  ∇𝑇  stands  for  Truesdell  rate.    This  expression  should  later  be 
identified with  
𝒇 ̇
mat =
int
mat
𝜕𝒇int
𝜕𝒖
𝒖̇ +
mat
𝜕𝒇int
𝜕𝑡
(22.62.7) 
in  order  to  determine  the  tangent  modulus.    Neglecting  discrepancies  between  the 
Jaumann and Truesdell rates, we can use (22.62.2) and (22.62.3) in (22.62.6) to get 
𝒇 ̇
mat = ∫ 𝑩𝑇 ∑(𝐾𝑚𝒊⨂𝒊 + 2𝐺𝑚𝑰dev)
int
𝑩𝑑𝛺 𝒖̇ − ∫ 𝑩𝑇 ∑(𝐾𝑚𝛽𝑚
𝑘 𝑡𝑚𝒊 + 2𝐺𝑚𝛽𝑚
𝑔 𝒔𝑚)
𝑑𝛺, (22.62.8) 
where  𝑰dev  is  the  4th  order  deviatoric  identity  tensor.  Comparing  this  expression  with 
(22.62.7) one can conclude that 
mat
𝜕𝒇int
𝜕𝒖
= ∫ 𝑩𝑇 ∑(𝐾𝑚𝒊⨂𝒊 + 2𝐺𝑚𝑰dev)
𝑩𝑑𝛺, 
and hence the tangent modulus is 
22-162 (Material Models)
LS-DYNA Theory Manual 
Material Models 
. 
𝑪 = ∑(𝐾𝑚𝒊⨂𝒊 + 2𝐺𝑚𝑰dev)
(22.62.10)
i.e., independent of deformation and time.  In fact, this tangent modulus is equal to the classical 
elastic tangent modulus for a hypoelastic material, cf. (22.62.4).  
22.62.4  Using the Relaxation Curve 
Instead of inputting the stiffness and relaxation parameters, one can input a relaxation 
curve  from  test  according  to  Figure  22.62.1.  The  time  scale  is  determined  by  BSTART 
and LS-DYNA will determine all parameters as to best fit the curve.
Material Models 
LS-DYNA Theory Manual 
22.63  Material Model 77:  Hyperviscoelastic Rubber  
Material  type  77  in  LS-DYNA  consists  of  two  hyperelastic  rubber  models,  a 
general hyperelastic rubber model and an Ogden rubber model, that can be combined 
optionally with a viscoelastic stress contribution.  As for the rate independent part, the 
constitutive  law  is  determined  by  a  strain  energy  function  which  in  this  case 
advantageously  can  be  expressed  in  terms  of  the  principal  stretches,  i.e.,  𝑊 =
𝑊(𝜆1, 𝜆2, 𝜆3).  To  obtain  the  Cauchy  stress  𝜎𝑖𝑗,  as  well  as  the  constitutive  tensor  of 
TC,  they  are  first  calculated  in  the  principal  basis  after  which  they  are 
interest,  𝐷𝑖𝑗𝑘𝑙
transformed back to the “base frame”, or standard basis.  The complete set of formulas 
is given by Crisfield [1997] and is for the sake of completeness recapitulated here. 
The principal Kirchoff stress components are given by 
E = 𝜆𝑖
𝜏𝑖𝑖
𝜕𝑊
𝜕𝜆𝑖
(no sum),
that are transformed to the standard basis using the standard formula 
E.
𝜏𝑖𝑗 = 𝑞𝑖𝑘𝑞𝑗𝑙𝜏𝑘𝑙
(22.63.1)
(22.63.2)
The 𝑞𝑖𝑗 are the components of the orthogonal tensor containing the eigenvectors 
of the principal basis.  The Cauchy stress is then given by  
𝜎𝑖𝑗 = 𝐽−1𝜏𝑖𝑗,
(22.63.3)
where 𝐽 = 𝜆1𝜆2𝜆3 is the relative volume change. 
The  constitutive  tensor  that  relates  the  rate  of  deformation  to  the  Truesdell 
(convected) rate of Kirchoff stress can in the principal basis be expressed as 
𝐷𝑖𝑖𝑗𝑗
TKE = 𝜆𝑗
TKE =
𝐷𝑖𝑗𝑖𝑗
TKE =
𝐷𝑖𝑗𝑖𝑗
E𝛿𝑖𝑗
− 2𝜏𝑖𝑖
𝜕𝜏𝑖𝑖
𝜕𝜆𝑗
2𝜏𝑗𝑗
E − 𝜆𝑖
2𝜏𝑖𝑖
𝜆𝑗
2 − 𝜆𝑗
𝜆𝑖
𝜕𝜏𝑖𝑖
(
𝜕𝜆𝑖
𝜆𝑖
−
𝜕𝜏𝑖𝑖
𝜕𝜆𝑗
),
𝑖 ≠ 𝑗, 𝜆𝑖 = 𝜆𝑗
,    𝑖 ≠ 𝑗, 𝜆𝑖 ≠ 𝜆𝑗
  (no sum). 
(22.63.4)
These components are transformed to the standard basis according to 
TK = 𝑞𝑖𝑝𝑞𝑗𝑞𝑞𝑘𝑟𝑞𝑙𝑠𝐷𝑝𝑞𝑟𝑠
TKE,
𝐷𝑖𝑗𝑘𝑙
(22.63.5)
and finally the constitutive tensor relating the rate of deformation to the Truesdell rate 
of Cauchy stress is obtained through
LS-DYNA Theory Manual 
Material Models 
𝐷𝑖𝑗𝑘𝑙
TC = 𝐽−1𝐷𝑖𝑗𝑘𝑙
TK .
(22.63.6)
When  dealing  with  shell  elements,  the  tangent  moduli  in  the  corotational 
coordinates is of interest.  This matrix is given by 
𝐷̂
TC = 𝑅𝑝𝑖𝑅𝑞𝑗𝑅𝑟𝑘𝑅𝑠𝑙𝐷𝑝𝑞𝑟𝑠
𝑖𝑗𝑘𝑙
TC = 𝐽−1𝑅𝑝𝑖𝑅𝑞𝑗𝑅𝑟𝑘𝑅𝑠𝑙𝐷𝑝𝑞𝑟𝑠
TK = 𝐽−1𝑞 ̂𝑖𝑝𝑞 ̂𝑗𝑞𝑞 ̂𝑘𝑟𝑞 ̂𝑙𝑠𝐷𝑝𝑞𝑟𝑠
TKE, 
(22.63.7)
where 𝑅𝑖𝑗 is the matrix containing the unit basis vectors of the corotational system and 
𝑞 ̂𝑖𝑗 = 𝑅𝑘𝑖𝑞𝑘𝑗. The latter matrix can be determined as the eigenvectors of the co-rotated left 
Cauchy-Green  tensor  (or  the  left  stretch  tensor).    In  LS-DYNA,  the  tangent  stiffness 
matrix is after assembly transformed back to the standard basis according to standard 
transformation formulae. 
22.63.1  General Hyperelastic Rubber Model 
The strain energy function for the general hyperelastic rubber model is given by 
𝑊 = ∑ 𝐶𝑝𝑞𝑊1
𝑝,𝑞=0
𝑝𝑊2
+
𝐾(𝐽 − 1)2,
where 𝐾 is the bulk modulus, 
−1
3 − 3
𝑊1 = 𝐼1𝐼3
−2/3 − 3,
𝑊2 = 𝐼2𝐼3
and 
𝐼1 = 𝜆1
𝐼2 = 𝜆1
𝐼3 = 𝜆1
2 + 𝜆2
2𝜆2
2𝜆2
2 + 𝜆2
2,
2𝜆3
2 + 𝜆3
2 + 𝜆1
2𝜆3
2 
2𝜆3
(22.63.8)
(22.63.9)
(22.63.10)
are  the  invariants  in  terms  of  the  principal  stretches.    To  apply  the  formulas  in  the 
previous section, we require 
E = 𝜆𝑖
𝜏𝑖𝑖
𝜕𝑊
𝜕𝜆𝑖
where 
= ∑ 𝐶𝑝𝑞(𝑝𝑊1
𝑝−1𝑊1𝑖
′ 𝑊2
𝑞 + 𝑞𝑊1
𝑝𝑊2
𝑞−1𝑊2𝑖
′ )
+ 𝐾𝐽(𝐽 − 1), 
(22.63.11)
𝑝,𝑞=0
𝑊1𝑖
′ ≔ 𝜆𝑖
𝑊2𝑖
′ : = 𝜆𝑖
𝜕𝑊1
𝜕𝜆𝑖
𝜕𝑊2
𝜕𝜆𝑖
= (2𝜆𝑖
2 −
−1
𝐼1) 𝐼3
= (2𝜆𝑖
2(𝐼1 − 𝜆𝑖
2) −
−2
3.
𝐼2) 𝐼3
(22.63.12)
If C𝑝𝑞 is nonzero only for 𝑝𝑞 = 01,10,11,20,02,30, then Equation (22.63.11) can be 
written as
Material Models 
LS-DYNA Theory Manual 
E = (𝐶10 + 𝐶11𝑊2 + 2𝐶20𝑊1 + 3𝐶30𝑊1
𝜏𝑖𝑖
         (𝐶01 + 𝐶11𝑊1 + 2𝐶02𝑊2)𝑊2𝑖
′ +
2)𝑊1𝑖
′ + 𝐾𝐽(𝐽 − 1).
(22.63.13)
Proceeding with the constitutive tensor, we have 
𝜆𝑗
𝜕𝜏𝑖𝑖
𝜕𝜆𝑗
𝑝,𝑞=0
= ∑ 𝐶𝑝𝑞(𝑝(𝑝 − 1)𝑊1
𝑝−2𝑊1𝑖
′ 𝑊1𝑗
′ 𝑊2
𝑞 + 𝑝𝑊1
𝑝−1𝑊1𝑖𝑗
′′ 𝑊2
𝑞 + 𝑝𝑞𝑊1
𝑝−1𝑊1𝑖
′ 𝑊2
𝑞−1𝑊2𝑗
′
𝑝−1𝑊1𝑗
+𝑞𝑝𝑊1
+𝐾𝐽(2𝐽 − 1),
′ 𝑊2
𝑞−1𝑊2𝑖
′ + 𝑞(𝑞 − 1)𝑊1
𝑝𝑊2
𝑞−2𝑊2𝑖
′ 𝑊2𝑗
′ + 𝑞𝑊1
𝑝𝑊2
𝑞−1𝑊2𝑖𝑗
′′ )
where 
𝑊1𝑖𝑗
′′ : = 𝜆𝑗
𝑊2𝑖𝑗
′′ : = 𝜆𝑗
′
𝜕𝑊1𝑖
𝜕𝜆𝑗
′
𝜕𝑊2𝑖
𝜕𝜆𝑗
= (4𝜆𝑖
2𝛿𝑖𝑗 −
(𝜆𝑖
2 + 𝜆𝑗
2) +
−1/3
𝐼1)𝐼3
= ((4𝜆𝑖
2𝐼1 − 8𝜆𝑖
4)𝛿𝑖𝑗 + 4𝜆𝑖
2𝜆𝑗
2 −
(𝜆𝑖
2(𝐼1 − 𝜆𝑖
2) + 𝜆𝑗
2(𝐼1 − 𝜆𝑗
2)) +
(22.63.14)
(22.63.15)
16
−2/3
𝐼2)𝐼3
Again, using only the nonzero coefficients mentioned above, Equation (22.63.14) 
is reduced to 
𝜆𝑗
𝜕𝜏𝑖𝑖
𝜕𝜆𝑗
= 𝐶11(𝑊1𝑖
′ 𝑊2𝑗
′ + 𝑊1𝑗
′ 𝑊2𝑖
′ ) + 2(𝐶20 + 3𝐶30𝑊1)𝑊1𝑗
′ 𝑊1𝑖
′ + 2𝐶02𝑊2𝑖
′ 𝑊2𝑗
′ +
(𝐶10 + 𝐶11𝑊2 + 2𝐶20𝑊1 + 3𝐶30𝑊1
𝐾𝐽(2𝐽 − 1).
2)𝑊1𝑖𝑗
′′ + (𝐶01 + 𝐶11𝑊1 + 2𝐶02𝑊2)𝑊2𝑖𝑗
′′ +
22.63.2  Ogden Rubber Model 
The strain energy function for the Ogden rubber model is given by  
𝑊 = ∑
𝑚=1
𝜇𝑚
𝛼𝑚
(𝜆̃
𝛼𝑚
+ 𝜆̃
𝛼𝑚 + 𝜆̃
𝛼𝑚 − 3) +
𝐾(𝐽 − 1)2,
where 
𝜆̃𝑖 =
𝜆𝑖
𝐽1/3,
  (22.63.16)
(22.63.17)
(22.63.18)
are  the  volumetric  independent  principal  stretches,  and  𝜇𝑚  and  𝛼𝑚  are  material 
parameters.  To apply the formulas in the previous section, we require 
E = 𝜆𝑖
𝜏𝑖𝑖
𝜕𝑊
𝜕𝜆𝑖
= ∑ 𝜇𝑚(𝜆̃
𝑚=1
𝛼𝑚 −
𝑎𝑚)
+ 𝐾𝐽(𝐽 − 1),
(22.63.19)
where 
22-166 (Material Models) 
𝑎𝑚 = 𝜆̃
𝛼𝑚 + 𝜆̃
𝛼𝑚 + 𝜆̃
𝛼𝑚.
LS-DYNA Theory Manual 
Material Models 
Proceeding with the constitutive tensor, we have 
𝜆𝑗
𝜕𝜏𝑖𝑖
𝜕𝜆𝑗
= ∑
𝑚=1
𝜇𝑚𝛼𝑚
(
𝑎𝑚 + 3𝜆̃
𝛼𝑚𝛿𝑖𝑗 − 𝜆̃
𝛼𝑚 − 𝜆̃
𝛼𝑚)
+ 𝐾𝐽(2𝐽 − 1). 
(22.63.21)
22.63.3  The Viscoelastic Contribution 
As  mentioned  above,  this  material  model  is  accompanied  with  a  viscoelastic 
stress  contribution.    The  rate  form  of  this  constitutive  law  can  in  co-rotational 
coordinates be written 
•
ve
𝜎̂𝑖𝑗
= ∑ 2𝐺𝑚
𝑚=1
𝐷̂ 𝑖𝑗
dev − ∑ 2𝛽𝑚𝐺𝑚 ∫ 𝑒−𝛽𝑚(𝑡−𝜏)𝐷̂ 𝑖𝑗
dev(𝜏)𝑑𝜏
.
(22.63.22)
𝑚=1
Here 𝑛 is a number less than or equal to 6, 𝜎̂𝑖𝑗
ve is the co-rotated viscoelastic stress, 
dev  is  the  deviatoric  co-rotated  rate-of-deformation  and  𝐺𝑚  and  𝛽𝑚  are  material 
𝐷̂ 𝑖𝑗
parameters.    The  parameters  𝐺𝑚  can  be  thought  of  as  shear  moduli  and  𝛽𝑚  as  decay 
coefficients determining the relaxation properties of the material.  This rate form can be 
integrated in time to form the corotated viscoelastic stress 
ve = ∑ 2𝐺𝑚 ∫ 𝑒−𝛽𝑚(𝑡−𝜏)𝐷̂ 𝑖𝑗
𝜎̂𝑖𝑗
𝑚=1
dev(𝜏)𝑑𝜏
.
(22.63.23)
For the constitutive matrix, we refer to Borrvall [2002] and here simply state that 
it is equal to 
𝐷̂
TCve = ∑ 2𝐺𝑚
𝑖𝑗𝑘𝑙
𝑚=1
(
(𝛿𝑖𝑘𝛿𝑗𝑙 + 𝛿𝑖𝑙𝛿𝑗𝑘) −
𝛿𝑖𝑗𝛿𝑘𝑙).
(22.63.24)
22.63.4  Stress Update for Shell Elements 
In principal, the stress update for material 77 and shell elements follows closely 
the  one  that  is  implemented  for  material  27.  The  stress  is  evaluated  in  corotational 
coordinates after which it is transformed back to the standard basis according to 
𝜎𝑖𝑗 = 𝑅𝑖𝑘𝑅𝑗𝑙𝜎̂𝑘𝑙,
(22.63.25)
or  equivalently  the  internal  force  is  assembled  in  the  corotational  system  and  then 
transformed back to the standard basis according to standard transformation formulae.  
Here 𝑅𝑖𝑗  is  the  rotation matrix  containing the corotational  basis  vectors.    The  so-called
Material Models 
LS-DYNA Theory Manual 
corotated stress 𝜎̂𝑖𝑗 is evaluated as the sum of the stresses given in Sections 19.77.1 and 
19.77.4.   
The  viscoelastic  stress  contribution  is  incrementally  updated  with  aid  of  the 
corotated  rate  of  deformation.    To  be  somewhat  more  precise,  the  values  of  the  12 
integrals  in  Equation  (22.63.23)  are  kept  as  history  variables  that  are  updated  in  each 
time  step.    Each  integral  is  discretized  in  time  and  the  mean  value  theorem  is  used  in 
each time step to determine their values.  
For  the  hyperelastic  stress  contribution,  the  principal  stretches  are  needed  and 
here  taken  as  the  square  root  of  the  eigenvalues  of  the  co-rotated  left  Cauchy-Green 
tensor 𝑏̂
𝑖𝑗. The corotated left Cauchy-Green tensor is incrementally updated with the aid 
of a time increment Δ𝑡, the corotated velocity gradient 𝐿̂ 𝑖𝑗, and the angular velocity 𝛺̂𝑖𝑗 
with which the embedded coordinate system is rotating,  
𝑖𝑗 = 𝑏̂
𝑏̂
𝑖𝑗 + Δ𝑡(𝐿̂ 𝑖𝑘 − 𝛺̂𝑖𝑘)𝑏̂
𝑘𝑗 + Δ𝑡𝑏̂
𝑖𝑘(𝐿̂ 𝑖𝑘 − 𝛺̂𝑖𝑘).
(22.63.26)
The  primary  reason  for  taking  a  corotational  approach  is  to  facilitate  the 
maintenance of a vanishing normal stress through the thickness of the shell, something 
that  is  achieved  by  adjusting  the  corresponding  component  of  the  corotated  velocity 
gradient  𝐿̂ 33  accordingly.    The  problem  can  be  stated  as  to  determine  L̂ 33  such  that 
when  updating  the  left  Cauchy-Green  tensor  through  Equation  (22.63.26)  and 
subsequently  the  stress  through  formulae  in  Sections  19.77.1  and  19.77.4,  𝜎̂33 = 0.  To 
this end, it is assumed that 
𝐿̂ 33 = α(𝐿̂ 11 + 𝐿̂ 22),
(22.63.27)
for some parameter α that is determined in the following three step procedure.  In the 
(0) 
first two steps, α = 0 and α = −1, respectively, resulting in two trial normal stresses 𝜎̂33
(−1).  Then  it  is  assumed  that  the  actual  normal  stress  depends  linearly  on  α, 
and  𝜎̂33
meaning that the latter can be determined from 
0 = 𝜎33
(α) = 𝜎33
(0) + α(𝜎33
(0) − 𝜎33
(−1)).
In the current implementation, α is given by 
(0)
𝜎̂33
(−1) − 𝜎̂33
𝜎̂33
(0)
if ∣𝜎̂33
(−1) − 𝜎̂33
(0)∣ ≥ 10−4
− 1
otherwise
𝛼 =
⎧
{
{
{
⎨
{
{
{
⎩
(22.63.28)
(22.63.29)
and  the  stresses  are  determined  from  this  value  of  𝛼.  Finally,  to  make  sure  that  the 
normal stress through the thickness vanishes, it is set to 0 (zero) before exiting the stress 
update routine.
LS-DYNA Theory Manual 
Material Models 
22.64  Material Model 78:  Soil/Concrete  
Concrete pressure is positive in compression.  Volumetric strain is defined as the 
natural  log  of  the  relative  volume  and  is  positive  in  compression  where  the  relative 
volume, 𝑉, is the ratio of the current volume to the initial volume.  The tabulated data 
should  be  given  in  order  of  increasing  compression.    If  the  pressure  drops  below  the 
cutoff  value  specified,  it  is  reset  to  that  value  and  the  deviatoric  stress  state  is 
eliminated. 
If  the  load  curve  ID  is  provided  as  a  positive  number,  the  deviatoric  perfectly 
plastic  pressure  dependent  yield  function  𝜙,  is  described  in  terms  of  the  second 
invariant, 𝐽2, the pressure, 𝑝, and the tabulated load curve, 𝐹(𝑝), as 
𝜙 = √3𝐽2 − 𝐹(𝑝) = σ𝑦 − 𝐹(𝑝),
where 𝐽2 is defined in terms of the deviatoric stress tensor as: 
assuming that if the ID is given as negative, then the yield function becomes: 
𝑆𝑖𝑗𝑆𝑖𝑗,
𝐽2 =
being the deviatoric stress tensor. 
𝜙 = 𝐽2 − 𝐹(𝑝),
(22.64.1)
(22.64.2)
(22.64.3)
If cracking is invoked, the yield stress is multiplied by a factor f which reduces 
with plastic stain according to a trilinear law as shown in Figure 22.64.1. 
1.0
Figure 22.64.1.  Strength reduction factor.
Material Models 
LS-DYNA Theory Manual 
Figure 22.64.2.  Cracking strain versus pressure. 
b = residual strength factor 
𝜀1 = plastic stain at which cracking begins. 
𝜀2 = plastic stain at which residual strength is reached. 
𝜀1 and 𝜀2 are tabulated functions of pressure that are defined by load curves .  The values on the curves are pressure versus strain and should be entered in 
order  of  increasing  pressure.    The  strain  values  should  always  increase  monotonically 
with pressure. 
By properly defining the load curves, it is possible to obtain the desired strength 
and ductility over a range of pressures.  See Figure 22.64.3.
Yield
stress
p3
p2
p1
Plastic strain
Figure 22.64.3.  Example Caption
LS-DYNA Theory Manual 
Material Models 
22.65  Material Model 79:  Hysteretic Soil 
This  model  is  a  nested  surface  model  with  five  superposed  “layers”  of  elasto-
perfectly  plastic  material,  each  with  its  own  elastic  modulii  and  yield  values.    Nested 
surface  models  give  hysteretic  behavior,  as  the  different  “layers”  yield  at  different 
stresses. 
The constants 𝑎0, 𝑎1, 𝑎2 govern the pressure sensitivity of the yield stress.  Only 
the ratios between these values are important - the absolute stress values are taken from 
the stress-strain curve.   
The stress strain pairs (𝛾1, 𝜏1), ... (𝛾5, 𝜏5) define a shear stress versus shear strain 
curve.  The first point on the curve is assumed by default to be (0,0) and does not need 
to  be  entered.    The  slope  of  the  curve  must  decrease  with  increasing  𝛾.    Not  all  five 
points  need  be  to  be  defined.    This  curve  applies  at  the  reference  pressure;  at  other 
pressures the curve varies according to 𝑎0, 𝑎1, and 𝑎2 as in the soil and crushable foam 
model, Material 5.  
The elastic moduli 𝐺 and 𝐾 are pressure sensitive. 
𝐺 = 𝐺0(𝑝 − 𝑝0)𝑏,
𝐾 = 𝐾0(𝑝 − 𝑝0)𝑏,
(22.65.1)
where  𝐺0  and  𝐾0  are  the  input  values,  𝑝  is  the  current  pressure,  𝑝0  the  cut-off  or 
reference pressure (must be zero or negative).  If 𝑝 attempts to fall below 𝑝0 (i.e., more 
tensile) the shear stresses are set to zero and the pressure is set to 𝑝0.  Thus, the material 
has  no  stiffness  or  strength  in  tension.    The  pressure  in  compression  is  calculated  as 
follows: 
where 𝑉 is the relative volume, i.e., the ratio between the original and current volume.
𝑝 = [−𝐾0ln(𝑉)]
1−𝑏⁄
,
(22.65.2)
Material Models 
LS-DYNA Theory Manual 
22.66  Material Model 80:  Ramberg-Osgood Plasticity 
The Ramberg-Osgood equation is an empirical constitutive relation to represent 
the  one-dimensional  elastic-plastic  behavior  of  many  materials,  including  soils.    This 
model  allows  a  simple  rate  independent  representation  of  the  hysteretic  energy 
dissipation  observed  in  soils  subjected  to  cyclic  shear  deformation.    For  monotonic 
loading, the stress-strain relationship is given by: 
𝛾𝑦
𝛾𝑦
=
=
𝜏𝑦
𝜏𝑦
+ 𝛼 ∣
− 𝛼 ∣
𝜏𝑦
𝜏𝑦
∣
∣
if  𝛾 ≥ 0,
if 𝛾 < 0,
(22.66.1)
where 𝛾 is the shear and 𝜏 is the stress.  The model approaches perfect plasticity as the 
stress  exponent  𝑟 → ∞.    These  equations  must  be  augmented  to  correctly  model 
unloading and reloading material behavior.  The first load reversal is detected by 𝛾𝛾̇ <
0.  After the first reversal, the stress-strain relationship is modified to  
(𝛾 − 𝛾0)
2𝛾𝑦
(𝛾 − 𝛾0)
2𝛾𝑦
=
=
(𝜏 − 𝜏0)
2𝜏𝑦
(𝜏 − 𝜏0)
2𝜏𝑦
+ 𝛼 ∣
− 𝛼 ∣
(𝜏 − 𝜏0)
∣
2𝜏𝑦
(𝜏 − 𝜏0)
∣
2𝜏𝑦
if 𝛾 ≥ 0,
if 𝛾 < 0,
(22.66.2)
where 𝛾0 and 𝜏0 represent the values of strain and stress at the point of load reversal.  
Subsequent load reversals are detected by (𝛾 − 𝛾0)𝛾̇ < 0. 
The  Ramberg-Osgood  equations  are  inherently  one-dimensional  and  are 
assumed  to  apply  to  shear  components.    To  generalize  this  theory  to  the  multidimen-
sional  case,  it  is  assumed  that  each  component  of  the  deviatoric  stress  and  deviatoric 
tensorial strain is independently related by the one-dimensional stress-strain equations.  
A projection is used to map the result back into deviatoric stress space if required.  The 
volumetric behavior is elastic, and, therefore, the pressure 𝑝 is found by  
𝑝 = −𝐾𝜀𝑣,
(22.66.3)
where 𝜀𝑣 is the volumetric strain.
LS-DYNA Theory Manual 
Material Models 
22.67  Material Models 81 and 82:  Plasticity with Damage 
and Orthotropic Option 
With  this  model  an  elasto-viscoplastic  material  with  an  arbitrary  stress  versus 
strain curve and arbitrary strain rate dependency can be defined.  Damage is considered 
before  rupture  occurs.    Also,  failure  based  on  a  plastic  strain  or  a  minimum  time  step 
size can be defined. 
An  option  in  the  keyword  input,  ORTHO,  is  available,  which  invokes  an 
orthotropic damage model.  This option is an extension to include orthotropic damage 
as  a  means  of  treating  failure  in  aluminum  panels.    Directional  damage  begins  after  a 
defined  failure  strain  is  reached  in  tension  and  continues  to  evolve  until  a  tensile 
rupture strain is reached in either one of the two orthogonal directions.   
The stress versus strain behavior may be treated by a bilinear stress strain curve 
by defining the tangent modulus, ETAN.  Alternately, a curve similar to that shown in 
Figure  22.67.1  is  expected  to  be  defined  by  (EPS1,ES1)  -  (EPS8,ES8);  however,  an 
effective stress versus effective plastic strain curve (LCSS) may be input instead if eight 
points  are  insufficient.    The  cost  is  roughly  the  same  for  either  approach.    The  most 
yield
yield stress versus
effective plastic strain
for undamaged material
Failure Begins
damage increases
linearly with plastic
strain after failure
nominal stress
after failure
rupture
ω=0
ω=1
εp
eff
Figure .22.67.1.  Stress strain behavior when damage is included. 
general approach is to use the table definition (LCSS) discussed below. 
Two  options  to  account  for  strain  rate  effects  are  possible.    Strain  rate  may  be 
accounted for using the Cowper-Symonds model which scales the yield stress with the 
factor,
Material Models 
LS-DYNA Theory Manual 
1 + (
𝑝⁄
)
,
𝜀̇
(22.67.1)
where 𝜀̇ is the strain rate, 𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗.  If the viscoplastic option is active, VP = 1.0, and if 
SIGY is > 0 then the dynamic yield stress is computed from the sum of the static stress, 
p ), which is typically given by a load curve ID, and the initial yield stress, SIGY, 
s(𝜀eff
𝜎y
multiplied by the Cowper-Symonds rate term as follows: 
𝜎𝑦(𝜀eff
p , 𝜀̇eff
p ) = 𝜎𝑦
s(𝜀eff
p ) + SIGY ⋅ (
p⁄
)
,
𝜀̇eff
(22.67.2)
where  the  plastic  strain  rate  is  used.    With  this  latter  approach  similar  results  can  be 
obtained 
model: 
model 
*MAT_ANISOTROPIC_VISCOPLASTIC.    If  SIGY = 0,  the  following  equation  is  used 
instead where the static stress, 𝜎y
p ), must be defined by a load curve: 
between 
material 
and 
this 
s(𝜀eff
𝜎y(𝜀eff
p , 𝜀̇eff
p ) = 𝜎y
p )
s(𝜀eff
𝜀̇eff
)
⎡
1 + (
⎢⎢
⎣
p⁄
⎤
. 
⎥⎥
⎦
(22.67.3)
This latter equation is always used if the viscoplastic option is off.  For complete 
generality  a  load  curve  (LCSR)  to  scale  the  yield  stress  may  be  input  instead.    In  this 
curve the scale factor versus strain rate is defined. 
The  constitutive  properties  for  the  damaged  material  are  obtained  from  the 
undamaged material properties.  The amount of damage evolved is represented by the 
constant,  𝜔,  which  varies  from  zero  if  no  damage  has  occurred  to  unity  for  complete 
rupture.  For uniaxial loading, the nominal stress in the damaged material is given by  
where P is the applied load and A is the surface area.  The true stress is given by:  
𝜎nominal =
,
(22.67.4)
𝜎true =
𝐴 − 𝐴loss
,
where 𝐴loss is the void area.  The damage variable can then be defined: 
𝜔 =
𝐴loss
,
0 ≤ 𝜔 ≤ 1.
(22.67.5)
(22.67.6)
In this model damage is defined in terms of plastic strain after the failure strain is 
exceeded: 
𝜔 =
p − 𝜀failure
𝜀eff
− 𝜀failure
𝜀rupture
    if    𝜀failure
≤ 𝜀eff
p ≤ 𝜀rupture
. 
(22.67.7)
LS-DYNA Theory Manual 
Material Models 
After  exceeding  the  failure  strain  softening  begins  and  continues  until  the 
rupture strain is reached. 
By  default,  deletion  of  a  shell  element occurs  when  all  integration  points  in  the 
shell  have  failed.    A  parameter  is  available,  NUMINT,  that  defines  the  number  of 
through  thickness  integration  points  for  shell  element  deletion.    The  default  of  all 
integration points is not recommended since shells undergoing large strain are often not 
deleted due to nodal fiber rotations which limit strains at active integration points after 
most points have failed.  Better results are obtained if NUMINT is set to 1 or a number 
less  than  one  half  of  the  number  of  through  thickness  points.    For  example,  if  four 
through  thickness  points  are  used,  NUMINT  should  not  exceed  2,  even  for  fully 
integrated shells which have 16 integration points. 
22.67.1  Material Model 82:  Isotropic Elastic-Plastic with Anisotropic Damage 
Material  82  is  an  isotropic  elastic-plastic  material  model  with  anisotropic 
damage..  The stress update in the case of shell elements is performed as follows.  For a 
𝑡,  𝑖 = 1, 2  at  time  𝑡,  the  local  stress  is 
given  stress  state  𝜎𝑖𝑗
obtained as  
𝑡   and  damage  parameters  𝐷𝑖
𝑡 ,
𝑙 = 𝑞𝑘𝑖𝑞𝑙𝑗𝜎𝑘𝑙
𝜎𝑖𝑗
(22.67.8)
where  𝑞𝑖𝑗  is  an  orthogonal  matrix  determining  the  direction  of  the  damage.    The 
directions are determined as follows.  The first direction is taken as the one in which the 
plastic strain first reaches the plastic strain at impending failure, see below.  The other 
direction is orthogonal to the first and in the plane of the shell. 
ε eff
p - f s
failure
Figure 22.67.2.  A nonlinear damage curve is optional.  Note that the origin of
the curve is at (0,0).  It is permissible to input the failure strain, fs, as zero for
this option.  The nonlinear damage curve is useful for controlling the softening
behavior after the failure strain is reached. 
For this local stress, the undamaged stress is computed as
Material Models 
LS-DYNA Theory Manual 
u =
𝜎11
u =
𝜎22
u =
𝜎12
u =
𝜎23
u =
𝜎13
t , 
𝜎11
1 − D1
𝜎22
𝑡 , 
1 − D2
2𝜎12
𝑡 , 
2 − 𝐷1
𝜎23
1 − 𝐷2
𝜎13
𝑡 .
1 − 𝐷1
𝑡 , 
𝑡 − 𝐷2
(22.67.9)
A  new  undamaged  stress  𝜎𝑖𝑗
u+  is  then  computed  following  a  standard  elastic-
plastic stress update.  The damage at the next time step is computed according to 
p − 𝜀f
𝜀𝑖𝑖
𝜀r − 𝜀f
𝑡+ = max (𝐷𝑖
𝑡,
𝑖 = 1, 2,
𝐷𝑖
) ,
(22.67.10)
where 𝜀f is the plastic strain at impending failure, 𝜀r is the plastic strain at rupture and 
p is the current plastic strain in the local 𝑖 direction.  There is also an option of defining 
𝜀𝑖𝑖
a nonlinear damage curve, with this option the new damage is computed as 
𝑡, 𝑓 (𝜀𝑖𝑖
𝑡+ = max(𝐷𝑖
p − 𝜀f)),
𝑖 = 1, 2,
(22.67.11)
𝐷𝑖
for a user-defined load curve 𝑓 . 
The new local (damaged) stress is given by  
l+ = 𝜎11
𝜎11
l+ = 𝜎22
𝜎22
l+ = 𝜎12
𝜎12
l+ = 𝜎23
𝜎23
l+ = 𝜎13
𝜎13
𝑡+),
u+(1 − 𝐷1
𝑡+), 
u+(1 − 𝐷2
t+
t+ − 𝐷2
u+ 2 − 𝐷1
t+), 
u+(1 − 𝐷2
t+),
u+(1 − 𝐷1
, 
(22.67.12)
which is transformed back to the local system to obtain the new global damaged stress 
as 
𝑙+.
𝑡+ = 𝑞𝑖𝑘𝑞𝑗𝑙𝜎𝑘𝑙
𝜎𝑖𝑗
(22.67.13)
An integration point is completely failed, i.e., it is removed from the calculations, 
when  max(𝐷1, 𝐷2) > 0.999.    The  element  is  removed  from  the  model  when  a  user 
specified number of integration points in that element have failed.
LS-DYNA Theory Manual 
Material Models 
There  are  options  of  using  visco-plasticity  in  the  current  model.    The  details  of 
this part of the stress update is omitted here. 
The Rc-Dc Damage Model 
The Rc-Dc model is defined as the following, see the report on the Fundamental 
Study of Crack Initiation and Propagation [2003].  The damage 𝐷 is updated as 
𝐷𝑡+ = 𝐷𝑡 + 𝜔1𝜔2Δ𝜀p
(22.67.14)
where Δ𝜀p is the plastic strain increment and 
𝜔1 = (1 + 𝛾𝑝)−𝛼,
𝜔2 = (2 − 𝐴𝐷)𝛽.
(22.67.15)
Here 𝑝 is the pressure, 𝛼, 𝛽 and 𝛾 are material parameters and 
𝐴𝐷 =
⎧
{{
⎨
{{
⎩
1.9999
if  max(𝑆1, 𝑆2) ≤ 0
min (∣
𝑆1
𝑆2
∣ , ∣
𝑆2
𝑆1
∣) otherwise
. 
(22.67.16)
where 𝑆1 and 𝑆2 are the in-plane principal stress values.  Fracture is initiated when the 
accumulation of damage is greater than a critical damage 𝐷c given by 
𝐷c = 𝐷0(1 + 𝑏‖∇𝐷‖𝜆).
(22.67.17)
Here 𝐷0, 𝑏 and λ are material parameters and ∇D is the spatial gradient of damage.  We 
have  added  an  option  to  use  a  non-local  formulation  with  𝐷  as  the  non-local  variable 
and  a  characteristic  length 𝑙.    More  information  on  this  can  be  found  in  the  LS-DYNA 
Keyword User’s Manual [Hallquist 2003].  With this option we compute 𝐷c as, 
𝐷c = 𝐷0,
(22.67.18)
hence the parameters 𝑏 and 𝜆 are not used.  A fracture fraction given by  
𝐹 =
𝐷 − 𝐷c
𝐷s
(22.67.19)
defines  the  degradations  of  the  material  by  the  Rc-Dc  model.    Here  𝐷s  is  yet  another 
parameter  determined  by  the  user.    The  stress  update  of  material  82  is  modified 
accordingly. 
Upon  entry  the  stress  is  divided  by  the  factor  1 − 𝐹𝑡  to  account  for  the  Rc-Dc 
damage.  Before exiting the routine, the stress is multiplied by the new Rc-Fc (reversed) 
fracture fraction 1 − 𝐹𝑡+. An integration point is considered failed when min(1 − 𝐷1, 1 −
𝐷2)(1 − 𝐹) < 0.001.
Material Models 
LS-DYNA Theory Manual 
22.68  Material Model 83:  Fu-Chang’s Foam With Rate 
Effects 
This model allows rate effects to be modeled in low and medium density foams, 
see Figure 22.68.1.  Hysteretic unloading behavior in this model is a function of the rate 
sensitivity with the most rate sensitive foams providing the largest hysteresis and visa 
versa.    The  unified  constitutive  equations  for  foam  materials  by  Fu-Chang  [1995] 
provide  the  basis  for  this  model.    This  implementation  incorporates  the  coding  in  the 
reference  in  modified  form  to  ensure  reasonable  computational  efficiency.    The 
mathematical description given below is excerpted from the reference. 
The  strain  is  divided  into  two  parts:  a  linear  part  and  a  non-linear  part  of  the 
strain   
and the strain rate becomes 
𝐄(𝑡) = 𝐄L(𝑡) + 𝐄N(𝑡),
𝐄̇(𝑡) = 𝐄̇L(𝑡) + 𝐄̇N(𝑡).
(22.68.1)
(22.68.2)
𝐄̇N is an expression for the past history of 𝐄N.  A postulated constitutive equation may 
be written as: 
Figure 22.68.1.  Rate effects in Fu Chang’s foam model. 
1-V
LS-DYNA Theory Manual 
Material Models 
∞
𝛔(𝑡) = ∫ [𝐄𝑡
N(𝜏), 𝐒(𝑡)]
𝑑𝜏,
𝜏=0
(22.68.3)
where 𝐒(𝑡) is the state variable and ∫
∞ and  
∞
𝜏=0  is a functional of all values of 𝜏 in 𝑇𝜏: 0 ≤ 𝜏 ≤
where 𝜏 is the history parameter: 
N(𝜏) = 𝐄N(𝑡 − 𝜏),
𝐄𝑡
N(𝜏 = ∞) ⇔ the virgin material.
𝐄𝑡
(22.68.4)
(22.68.5)
It  is  assumed  that  the  material  remembers  only  its  immediate  past,  i.e.,  a 
N(𝜏) in a Taylor series about 
neighborhood about 𝜏 = 0.  Therefore, an expansion of 𝐄𝑡
𝜏 = 0 yields: 
N(𝜏) = 𝐄N(0) +
𝐄𝑡
𝜕𝐄𝑡
𝜕𝑡
(0)𝑑𝑡.
Hence, the postulated constitutive equation becomes: 
𝛔(𝑡) = 𝛔∗(𝐄N(𝑡), 𝐄̇N(𝑡), 𝐒(𝑡)),
where we have replaced 
∂𝐄𝑡
∂𝑡  by 𝐄̇N, and 𝛔∗ is a function of its arguments. 
For a special case,  
we may write 
𝛔(𝑡) = 𝛔∗(𝐄̇N(𝑡), 𝐒(𝑡)),
N = 𝑓 (𝐒(𝑡), 𝐬(𝑡)),
𝐄̇𝑡
(22.68.6)
(22.68.7)
(22.68.8)
(22.68.9)
which  states  that  the nonlinear  strain  rate  is  the  function  of  stress  and  a  state  variable 
which  represents  the  history  of  loading.    Therefore,  the  proposed  kinetic  equation  for 
foam materials is: 
𝐄̇N =
‖𝛔‖
𝐷0exp [−𝑐0 (
2𝑛0
tr(𝛔𝐒)
(‖𝛔‖)2 )
],
(22.68.10)
where 𝐷0, 𝑐0, and 𝑛0 are material constants, and 𝐒 is the overall state variable.  If either 
𝐷0 = 0 or 𝑐0 → ∞ then the nonlinear strain rate vanishes. 
𝑆̇𝑖𝑗 = [𝑐1(𝑎𝑖𝑗𝑅 − 𝑐2𝑆𝑖𝑗)𝑃 + 𝑐3𝑊𝑛1(∥𝐸̇𝑁∥)
𝑛2𝐼𝑖𝑗]𝑅
𝑅 = 1 + 𝑐4
𝑛3
∥𝐄̇N∥
𝑐5
⎜⎛
⎝
− 1
⎟⎞
⎠
𝑃 = tr(𝛔𝐄̇N)
(22.68.11)
(22.68.12)
(22.68.13)
Material Models 
LS-DYNA Theory Manual 
where 𝑐1, 𝑐2, 𝑐3, 𝑐4, 𝑐5, 𝑛1, 𝑛2, 𝑛3, and 𝑎𝑖𝑗 are material constants and: 
W = ∫ tr(𝛔𝑑𝐄),
(22.68.14)
2,
‖𝛔‖ = (𝜎𝑖𝑗𝜎𝑖𝑗)
∥𝐄̇∥ = (𝐸̇𝑖𝑗𝐸̇𝑖𝑗)
2, 
N)
2.
∥𝐄̇N∥ = (𝐸̇𝑖𝑗
N𝐸̇𝑖𝑗
(22.68.15)
In the implementation by Fu Chang the model was simplified such that the input 
constants 𝑎𝑖𝑗 and the state variables 𝑆𝑖𝑗 are scalars. 
Viscous  damping  in  the  model  follows  an  implementation  identical  to  that  of 
material type 57.
LS-DYNA Theory Manual 
Material Models 
22.69  Material Model 84 and 85:  Winfrith Concrete 
Pressure is positive in compression; volumetric strain is given by the natural log 
of the relative volume and is negative in compression.  The tabulated data are given in 
order of increasing compression, with no initial zero point. 
If  the  volume  compaction  curve  is  omitted,  the  following  scaled  curve  is 
automatically  used  where  𝑝1  is  the  pressure  at  uniaxial  compressive  failure  computed 
from: 
𝑝1 =
𝜎𝑐
,
and 𝐾 is the unloading bulk modulus computed from 
𝐾 =
𝐸s
,
3(1 − 2𝑣)
where 𝐸s is the input tangent modulus for concrete and 𝑣 is Poisson's ratio. 
(22.69.1)
(22.69.2)
Volumetric Strain
−𝑝1/K
-0.002 
-0.004 
-0.010 
-0.020 
-0.030 
-0.041 
-0.051 
-0.062 
-0.094 
Pressure (MPa) 
1.00 × 𝑝1
1.50 × 𝑝1
3.00 × 𝑝1
4.80 × 𝑝1
6.00 × 𝑝1
7.50 × 𝑝1
9.45 × 𝑝1
11.55 × 𝑝1
14.25 × 𝑝1
25.05 × 𝑝1
Table 22.3. Default pressure versus volumetric strain curve for concrete if the curve is 
not defined.
Material Models 
LS-DYNA Theory Manual 
22.70  Material Model 87:  Cellular Rubber 
This  material  model  provides  a  cellular  rubber  model  combined  with  linear 
viscoelasticity as outlined by Christensen [1980]. 
Rubber is generally considered to be fully incompressible since the bulk modulus 
greatly  exceeds  the  shear  modulus  in  magnitude.    To  model  the  rubber  as  an 
unconstrained material a hydrostatic work term, 𝑊𝐻(𝐽), is included in the strain energy 
functional which is function of the relative volume, 𝐽, [Ogden, 1984]: 
𝑊(𝐽1, 𝐽2, 𝐽) = ∑ 𝐶𝑝𝑞
(𝐽1 − 3)𝑝(𝐽2 − 3)𝑞 + 𝑊𝐻(𝐽)
𝑝,𝑞=0
 −1
3⁄
𝐽1 = 𝐼1𝐼3
𝐽2 = 𝐼2𝐼3
 −2
3⁄
(22.70.1)
In  order  to  prevent  volumetric  work  from  contributing  to  the  hydrostatic  work 
the first and second invariants are modified as shown.  This procedure is described in 
more detail by Sussman and Bathe [1987]. 
The  effects  of  confined  air  pressure  in  its  overall  response  characteristics  are 
included by augmenting the stress state within the element by the air pressure. 
𝜎𝑖𝑗 = 𝜎𝑖𝑗
sk − 𝛿𝑖𝑗𝜎 air,
(22.70.2)
sk  is  the  bulk  skeletal  stress  and  σair  is  the  air  pressure  computed  from  the 
where  𝜎𝑖𝑗
equation: 
𝜎 air = −
𝑝0𝛾
1 + 𝛾 − 𝜙
,
(22.70.3)
where 𝑝0  is  the  initial  foam  pressure  usually  taken  as  the  atmospheric  pressure  and  𝛾 
defines the volumetric strain  
where 𝑉 is the relative volume of the voids and 𝛾0 is the initial volumetric strain which 
is typically zero.  The rubber skeletal material is assumed to be incompressible. 
𝛾 = 𝑉 − 1 + 𝛾0,
(22.70.4)
Rate effects are taken into account through linear viscoelasticity by a convolution 
integral of the form: 
𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙
(𝑡 − 𝜏)
𝜕𝜀𝑘𝑙
𝜕𝜏
𝑑𝜏,
(22.70.5)
or in terms of the second Piola-Kirchhoff stress, 𝑆𝑖𝑗, and Green's strain tensor, 𝐸𝑖𝑗,
LS-DYNA Theory Manual 
Material Models 
𝑆𝑖𝑗 = ∫ 𝐺𝑖𝑗𝑘𝑙
(𝑡 − 𝜏)
𝜕𝐸𝑘𝑙
𝜕𝜏
𝑑𝜏,
(22.70.6)
where  𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)  and  𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏)  are  the  relaxation  functions  for  the  different  stress 
measures.    This  stress  is  added  to  the  stress  tensor  determined  from  the  strain  energy 
functional.   
Since  we  wish  to  include  only  simple  rate  effects,  the  relaxation  function  is 
represented by one term from the Prony series: 
given by, 
𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚
𝑚=1
𝑒−𝛽𝑡,
𝑔(𝑡) = 𝐸𝑑𝑒−𝛽1𝑡.
(22.70.7)
(22.70.8)
This model is effectively a Maxwell fluid which consists of a damper and spring 
in series.  We characterize this in the input by a shear modulus, 𝐺, and decay constant, 
𝛽1.   
The Mooney-Rivlin rubber model is obtained by specifying 𝑛 = 1.  In spite of the 
differences  in  formulations  with  Model  27,  we  find  that  the  results  obtained  with  this 
model are nearly identical with those of 27 as long as large values of Poisson’s ratio are 
used.
Rubber Block with Entrapped Air
Air
Figure  22.70.1.   Cellular rubber  with entrapped  air.  By setting the initial air
pressure to zero, an open cell, cellular rubber can be simulated.
Material Models 
LS-DYNA Theory Manual 
22.71  Material Model 88:  MTS Model 
The  Mechanical  Threshhold  Stress  (MTS)  model  is  due  to  Mauldin,  Davidson, 
and  Henninger  [1990]  and  is  available  for  applications  involving  large  strains,  high 
pressures and strain rates.  As described in the foregoing reference, this model is based 
on  dislocation  mechanics  and  provides  a  better  understanding  of  the  plastic 
deformation process for ductile materials by using an internal state variable called the 
mechanical  threshold  stress.    This  kinematic  quantity  tracks  the  evolution  of  the 
material’s  microstructure  along  some  arbitrary  strain,  strain  rate,  and  temperature-
dependent  path  using  a  differential  form  that  balances  dislocation  generation  and 
recovery processes.  Given a value for the mechanical threshold stress, the flow stress is 
determined  using  either  a  thermal-activation-controlled  or  a  drag-controlled  kinetics 
relationship.    An  equation-of-state  is  required  for  solid  elements  and  a  bulk  modulus 
must be defined below for shell elements. 
The flow stress 𝜎 is given by: 
𝜎 = 𝜎̂a +
𝐺0
[𝑠th𝜎̂ + 𝑠th,𝑖𝜎̂𝑖 + 𝑠th,𝑠𝜎̂s].
(22.71.1)
The first product in the equation for 𝜎 contains a micro-structure evolution variable, i.e., 
𝜎̂ ,  called  the  Mechanical  Threshold  Stress  (MTS),  that  is  multiplied  by  a  constant-
structure  deformation  variable  𝑠th:𝑠th  is  a  function  of  absolute  temperature  𝑇  and  the 
plastic  strain-rates  𝜀̇P.    The  evolution  equation  for  𝜎̂   is  a  differential  hardening  law 
representing dislocation-dislocation interactions: 
∂σ̂
∂𝜀p ≡ Θo
1 −
⎡
⎢
⎢
⎢
⎣
tanh (α σ̂
𝜎̂εs
tanh(𝛼)
)
. 
⎤
⎥
⎥
⎥
⎦
(22.71.2)
The  term,  ∂𝜎̂
∂𝜀p,  represents  the  hardening  due  to  dislocation  generation  and  the 
stress ratio,  𝜎̂
, represents softening due to dislocation recovery.  The threshold stress at 
𝜎̂εs
zero strain-hardening 𝜎̂εs is called the saturation threshold stress.  Relationships for 𝛩𝑜, 
𝜎̂εs are: 
𝛩𝑜 = 𝑎𝑜 + 𝑎1ln (
𝜀̇p
𝜀0
) + 𝑎2√
𝜀̇p
𝜀0
,
(22.71.3)
which contains the material constants 𝑎o, 𝑎1, and 𝑎2.  The constant, 𝜎̂εs, is given as: 
𝜎̂εs = 𝜎̂εso (
𝑘𝑇/𝐺𝑏3𝐴
,
𝜀̇𝑝
𝜀̇εso
)
(22.71.4)
LS-DYNA Theory Manual 
Material Models 
which  contains  the  input  constants:  𝜎̂εso,  𝜀̇εso,  𝑏,  𝐴,  and  𝑘.    The  shear  modulus  𝐺 
appearing in these equations is assumed to be a function of temperature and is given by 
the correlation. 
𝐺 = 𝐺0 −
𝑏1
,
𝑏2
𝑇 − 1
which  contains  the  constants:  𝐺0,  𝑏1,  and  𝑏2.    For  thermal-activation  controlled 
deformation 𝑠th is evaluated via an Arrhenius rate equation of the form: 
(22.71.5)
⎜⎜⎜⎜⎜⎛𝑘𝑇ln (
𝐺𝑏3𝑔0
𝜀̇0
𝜀̇p)
⎟⎟⎟⎟⎟⎞
𝑠th =
1 −
⎡
⎢
⎢
⎢
⎢
⎣
⎝
⎤
⎥
⎥
⎥
⎥
⎦
. 
(22.71.6)
⎠
The absolute temperature is given as: 
where 𝐸 in the internal energy density per unit initial volume.
𝑇 = 𝑇ref + 𝜌𝑐p𝐸,
(22.71.7)
Material Models 
LS-DYNA Theory Manual 
22.72  Material Model 89:  Plasticity Polymer 
Unlike  other  LS-DYNA  material  models,  both  the  input  stress-strain  curve  and 
the strain to failure are defined as total true strain, not plastic strain.  The input can be 
defined  from  uniaxial  tensile  tests;  nominal  stress  and  nominal  strain  from  the  tests 
must be converted to true stress and true strain.  The elastic component of strain must 
not be subtracted out. 
The stress-strain curve is permitted to have sections steeper (i.e. stiffer) than the 
elastic  modulus.    When  these  are  encountered  the  elastic  modulus  is  increased  to 
prevent spurious energy generation.
LS-DYNA Theory Manual 
Material Models 
22.73  Material Model 90:  Acoustic 
This  model  is  appropriate  for  tracking  low-pressure  stress  waves  in  an  acoustic 
media  such  as  air  or  water  and  can  be  used  only  with  the  acoustic  pressure  element 
formulation.  The acoustic pressure element requires only one unknown per node.  This 
element is very cost effective.
Material Models 
LS-DYNA Theory Manual 
22.74  Material Model 91:  Soft Tissue 
The overall strain energy W is "uncoupled" and includes two isotropic deviatoric 
matrix terms, a fiber term F, and a bulk term: 
𝑊 = 𝐶1(𝐼 ̃1 − 3) + 𝐶2(𝐼 ̃2 − 3) + 𝐹(𝜆) +
𝐾[ln(𝐽)]2.
(22.74.1)
Here, 𝐼 ̃1 and 𝐼 ̃2 are the deviatoric invariants of the right Cauchy deformation tensor, 𝜆 is 
the  deviatoric  part  of  the  stretch  along  the  current  fiber  direction,  and  𝐽 = det𝐅  is  the 
volume  ratio.    The  material  coefficients  𝐶1  and  𝐶2  are  the  Mooney-Rivlin  coefficients, 
while 𝐾 is the effective bulk modulus of the material (input parameter XK). 
The derivatives of the fiber term 𝐹 are defined to capture the behavior of crimped 
collagen.  The fibers are assumed to be unable to resist compressive loading - thus the 
model is isotropic when 𝜆 < 1.  An exponential function describes the straightening of 
the  fibers,  while  a  linear  function  describes  the  behavior  of  the  fibers  once  they  are 
straightened past a critical fiber stretch level 𝜆 ≥ 𝜆∗ (input parameter XLAM): 
∂𝐹
∂λ
=
⎧0
{{{
𝐶3
⎨
{{{
⎩
𝜆 < 1
[exp(𝐶4(𝜆 − 1)) − 1] 𝜆 < 𝜆∗
. 
(22.74.2)
(𝐶5𝜆 + 𝐶6)
𝜆 ≥ 𝜆∗
Coefficients 𝐶3, 𝐶4, and 𝐶5 must be defined by the user.  𝐶6 is determined by LS-DYNA 
to ensure stress continuity at 𝜆 = 𝜆∗.  Sample values for the material coefficients 𝐶1 − 𝐶5 
and 𝜆∗ for ligament tissue can be found in Quapp and Weiss [1998].  The bulk modulus 
K should be at least 3 orders of magnitude larger than 𝐶1 to ensure near-incompressible 
material behavior. 
Viscoelasticity is included via a convolution integral representation for the time-
dependent second Piola-Kirchoff stress 𝐒(𝐂, 𝑡): 
𝐒(𝐂, 𝑡) = 𝐒e(𝐂) + ∫ 2𝐺(𝑡 − 𝑠)
∂W
∂𝐂(s)
𝑑𝑠.
(22.74.3)
Here, 𝐒e is the elastic part of the second PK stress as derived from the strain energy, and 
𝐺(𝑡 − 𝑠) is the reduced relaxation function, represented by a Prony series: 
𝐺(t) = ∑ S𝑖
𝑖=1
exp (
𝑇𝑖
).
(22.74.4)
Puso and Weiss [1998] describe a graphical method to fit the Prony series coefficients to 
relaxation  data  that  approximates  the  behavior  of  the  continuous  relaxation  function 
proposed by Y-C. Fung, as quasilinear viscoelasticity.
LS-DYNA Theory Manual 
Material Models 
22.75  Material Model 94:  Inelastic Spring Discrete Beam 
The yield force is taken from the load curve: 
𝐹Y = 𝐹y(Δ𝐿plastic),
where 𝐿plastic is the plastic deflection.  A trial force is computed as: 
and is checked against the yield force to determine F: 
𝐹T = 𝐹n + 𝐾 ⋅ Δ𝐿̇ ⋅ Δ𝑡,
𝐹 = {𝐹Y if 𝐹T > 𝐹Y
𝐹T if 𝐹T ≤ 𝐹Y.
(22.75.1)
(22.75.2)
(22.75.3)
The final force, which includes rate effects and damping, is given by: 
𝐹𝑛+1 = 𝐹 ⋅ [1 + 𝐶1 ⋅ Δ𝐿̇ + 𝐶2 ⋅ sgn(Δ𝐿̇)ln (max {1. ,
∣Δ𝐿̇∣
DLE
})] + DΔ𝐿̇ + 𝑔(𝛥𝐿)ℎ(𝛥𝐿̇), (22.75.4)
where 𝐶1, 𝐶2 are damping coefficients, DLE is a factor to scale time units.   
Unless the origin of the curve starts at (0,0), the negative part of the curve is used 
when the spring force is negative where the negative of the plastic displacement is used 
to interpolate, 𝐹y.  The positive part of the curve is used whenever the force is positive.  
In these equations, Δ𝐿 is the change in length  
Δ𝐿 = current  length-initial  length.
(22.75.5)
Material Models 
LS-DYNA Theory Manual 
22.76  Material Model 96:  Brittle Damage Model 
A full description of the tensile and shear damage parts of this material model is 
given in Govindjee, Kay and Simo [1994,1995].  It is an anisotropic brittle damage model 
designed  primarily  for  concrete,  though  it  can  be  applied  to  a  wide  variety  of  brittle 
materials.    It  admits  progressive  degradation  of  tensile  and  shear  strengths  across 
smeared  cracks  that  are  initiated  under  tensile  loadings.    Compressive  failure  is 
governed by a simplistic J2 flow correction that can be disabled if not desired.  Damage 
is handled by treating the rank 4 elastic stiffness tensor as an evolving internal variable 
for the material.  Softening induced mesh dependencies are handled by a characteristic 
length method [Oliver 1989]. 
Description of properties: 
1. 
2. 
3. 
𝐸 is the Young's modulus of the undamaged material also known as the virgin 
modulus. 
𝜐  is  the  Poisson's  ratio  of  the  undamaged  material  also  known  as  the  virgin 
Poisson's ratio. 
𝑓𝑛  is  the  initial  principal  tensile  strength  (stress)  of  the  material.    Once  this 
stress has been reached at a point in the body a smeared crack is initiated there 
with a normal that is co-linear with the 1st principal direction.  Once initiated, 
the crack is fixed at that location, though it will convect with the motion of the 
body.    As  the  loading  progresses  the  allowed  tensile  traction  normal  to  the 
crack plane is progressively degraded to a small machine dependent constant.  
The degradation is implemented by reducing the material's modulus normal to 
the smeared crack plane according to a maximum dissipation law that incorpo-
rates exponential softening.  The restriction on the normal tractions is given by 
𝜙t = (𝐧 ⊗ 𝐧): 𝛔 − 𝑓n + (1 − 𝜀)𝑓n(1 − exp[−𝐻𝛼]) ≤ 0,
(22.76.1)
where 𝐧 is the smeared crack normal, 𝜀 is the small constant, 𝐻 is the softening 
modulus, and 𝛼 is an internal variable.  𝐻 is set automatically by the program; 
see 𝑔c below.  𝛼 measures the crack field intensity and is output in the equiva-
lent plastic strain field, 𝜀̅p, in a normalized fashion. 
The  evolution  of  alpha  is  governed  by  a  maximum  dissipation  argument.  
When the normalized value reaches unity it means that the material's strength 
has  been  reduced  to  2%  of  its  original  value  in  the  normal  and  parallel  direc-
tions to the smeared crack.  Note that for plotting purposes, it is never output 
greater than 5.
LS-DYNA Theory Manual 
Material Models 
4. 
5. 
6. 
7. 
8. 
𝑓s  is  the  initial  shear  traction  that  may  be  transmitted  across  a  smeared  crack 
plane.    The  shear  traction  is  limited  to  be  less  than  or  equal  to  𝑓s(1 − 𝛽)(1 −
exp[−𝐻𝛼]),  through  the  use  of  two  orthogonal  shear  damage  surfaces.    Note 
that  the  shear  degradation  is  coupled  to  the  tensile  degradation  through  the 
internal variable alpha which measures the intensity of the crack field. 𝛽 is the 
shear retention factor defined below.  The shear degradation is taken care of by 
reducing the material's shear stiffness parallel to the smeared crack plane. 
𝑔c  is  the  fracture  toughness  of  the  material.    It  should  be  entered  as  fracture 
energy  per  unit  area  crack  advance.    Once  entered  the  softening  modulus  is 
automatically calculated based on element and crack geometries.  
𝛽  is  the  shear  retention  factor.    As  the  damage  progresses  the  shear  tractions 
allowed across the smeared crack plane asymptote to the product 𝛽𝑓s. 
𝜂 represents the viscosity of the material.  Viscous behavior is implemented as 
a simple Perzyna regularization method.  This allows for the inclusion of first 
order rate effects.  The use of some viscosity is recommend as it serves as regu-
larizing parameter that increases the stability of calculations. 
𝜎y  is  a  uniaxial  compressive  yield  stress.    A  check  on  compressive  stresses  is 
made using the J2 yield function s: s − √2
3 𝜎y ≤ 0, where s is the stress deviator.  
If violated, a J2 return mapping correction is executed.  This check is executed 
when  (1)  no  damage  has  taken  place  at  an  integration  point  yet,    (2)  when 
damage  has  taken  place  at  a  point  but  the  crack  is  currently  closed,  and  (3) 
during  active  damage  after  the  damage  integration  (ie.    as  an  operator  split).  
Note  that  if  the  crack  is  open,  the  plasticity  correction  is  done  in  the  plane-
stress subspace of the crack plane. 
Remark:    A  variety  of  experimental  data  has  been  replicated  using  this  model 
from  quasi-static  to  explosive  situations.    Reasonable  properties  for  a  standard  grade 
concrete would be  𝐸 = 3.15 × 106psi, 𝑓n = 450 psi, 𝑓s = 2100 psi, 𝑣 = 0.2, 𝑔c = 0.8 lbs/in, 
𝛽 = 0.03,  𝜂 = 0.0 psi-sec,  𝜎y = 4200 psi.    For  stability,  values  of  𝜂  between  104  to  106 
psi/sec  are  recommended.    Our  limited  experience  thus  far  has  shown  that  many 
problems require nonzero values of 𝜂 to run to avoid error terminations.  Various other 
internal  variables  such  as  crack  orientations  and  degraded  stiffness  tensors  are 
internally calculated but currently not available for output.
Material Models 
LS-DYNA Theory Manual 
22.77  Material Model 97:  General Joint Discrete Beam 
For  explicit  calculations,  the  additional  stiffness  due  to  this  joint  may  require 
additional mass and inertia for stability.  Mass and rotary inertia for this beam element 
is  based  on  the  defined  mass  density,  the  volume,  and  the  mass  moment  of  inertia 
defined in the *SECTION_ BEAM input. 
The  penalty  stiffness  applies  to  explicit  calculations.    For  implicit  calculations, 
constraint  equations  are  generated  and  imposed  on  the  system  equations;  therefore, 
these constants, RPST and RPSR, are not used.
LS-DYNA Theory Manual 
Material Models 
22.78  Material Model 98:  Simplified Johnson Cook 
Johnson and Cook express the flow stress as 
𝜎𝑦 = (𝐴 + 𝐵𝜀̅
p𝑛
) (1 + 𝐶ln𝜀̇∗),
(22.78.1)
where  
𝐴, 𝐵, 𝐶 and 𝑛 are input constants 
𝜀̅p effective plastic strain 
𝜀̇∗ = 𝜀̅
𝜀̇0
 effective strain rate for 𝜀̇0 = 1s−1 
The maximum stress is limited by SIGMAX and SIGSAT by: 
𝜎y = min {min [𝐴 + 𝐵𝜀̅
p𝑛
, SIGMAX] (1 + 𝐶ln𝜀̇∗), SIGSAT}. 
(22.78.2)
Failure occurs when the effective plastic strain exceeds PSFAIL.     
If the viscoplastic option is active, VP = 1.0, the parameters SIGMAX and SIGSAT 
are ignored since these parameters make convergence of the viscoplastic strain iteration 
loop  difficult  to  achieve.    The  viscoplastic  option  replaces  the  plastic  strain  in  the 
forgoing equations by the viscoplastic strain and the strain rate by the viscoplastic strain 
rate.  Numerical noise is substantially reduced by the viscoplastic formulation.
LS-DYNA Draft
Material Models 
LS-DYNA Theory Manual 
22.79  Material Model 100:  Spot Weld 
This material model applies to beam element type 9 for spot welds.  These beam 
elements may be placed between any two deformable shell surfaces, see Figure 22.79.1, 
and  tied  with  type  7  constraint  contact  which  eliminates  the  need  to  have  adjacent 
nodes at spot weld locations.  Beam spot welds may be placed between rigid bodies and 
rigid/deformable bodies by making the node on one end of the spot weld a rigid body 
node which can be an extra node for the rigid body.   In the same way, rigid bodies may 
also be tied together with this spot weld option.  
It is advisable to include all spot welds, which provide the slave nodes, and spot 
welded  materials,  which  define  the  master  segments,  within  a  single  type  7  tied 
interface.  As a constraint method, multiple type 7 interfaces are treated independently 
which  can  lead  to  significant  problems  if  such  interfaces  share  common  nodal  points.  
The offset option, “o 7”, should not be used with spot welds. 
The  DAMAGE-FAILURE  option  causes  one  additional  line  to  be  read  with  the 
damage  parameter  and  a  flag  that  determines  how  failure  is  computed  from  the 
resultants.    On  this  line  the  parameter,  DMG,  if  nonzero,  invokes  damage  mechanics 
combined with the plasticity model to achieve a smooth drop off of the resultant forces 
prior  to  the  removal  of  the  spot  weld.    The  parameter  FOPT  determines  the  method 
used in computing resultant based failure, which is unrelated to damage. 
The weld material is modeled with isotropic hardening plasticity coupled to two 
failure  models.    The  first  model  specifies  a  failure  strain  which  fails  each  integration 
SPOTWELD ELEMENT
Trr
Frr
Mtt
Mss
Frt
Frs
n2
n1
Figure  22.79.1.    Deformable  spotwelds  can  be  arbitrarily  placed  within  the
structure.
LS-DYNA Theory Manual 
Material Models 
point  in  the  spot  weld  independently.    The  second  model  fails  the  entire  weld  if  the 
resultants are outside of the failure surface defined by: 
(
𝑁𝑟𝑟
𝑁𝑟𝑟F
)
+ (
𝑁𝑟𝑠
𝑁𝑟𝑠F
)
+ (
𝑁𝑟𝑡
𝑁𝑟𝑡F
)
+ (
𝑀𝑟𝑟
𝑀𝑟𝑟F
)
+ (
𝑀𝑠𝑠
𝑀𝑠𝑠F
)
+ (
𝑇𝑟𝑟
𝑇𝑟𝑟F
)
− 1 = 0, 
(22.79.1)
where  the  numerators  in  the  equation  are  the  resultants  calculated  in  the  local 
coordinates  of  the  cross  section,  and  the  denominators  are  the  values  specified  in  the 
input.  If the user defined parameter, NF, which the number of force vectors stored for 
filtering,  is  nonzero  the  resultants  are  filtered  before  failure  is  checked.    The  default 
value is set to zero which is generally recommended unless oscillatory resultant forces 
are  observed  in  the  time  history  databases.    Even  though  these  welds  should  not 
oscillate  significantly,  this  option  was  added  for  consistency  with  the  other  spot  weld 
options.    NF  affects  the  storage  since  it  is  necessary  to  store  the  resultant  forces  as 
history variables.   
If the failure strain is set to zero, the failure strain model is not used.  In a similar 
manner, when the value of a resultant at failure is set to zero, the corresponding term in 
the failure surface is ignored.  For example, if only N𝑟𝑟F is nonzero, the failure surface is 
reduced  to  |N𝑟𝑟| = N𝑟𝑟F.    None,  either,  or  both  of  the  failure  models  may  be  active 
depending on the specified input values.  
The  inertias  of  the  spot  welds  are  scaled  during  the  first  time  step  so  that  their 
stable time step size is Δ𝑡.  A strong compressive load on the spot weld at a later time 
may reduce the length of the spot weld so that stable time step size drops below Δ𝑡. If 
the value of Δ𝑡 is zero, mass scaling is not performed, and the spot welds will probably 
limit  the  time  step  size.    Under  most  circumstances,  the  inertias  of  the  spot  welds  are 
small enough that scaling them will have a negligible effect on the structural response 
and the use of this option is encouraged. 
Spotweld  force  history  data  is  written  into  the  SWFORC  ASCII  file.    In  this 
database the resultant moments are not available, but they are in the binary time history 
database. 
The  constitutive  properties  for  the  damaged  material  are  obtained  from  the 
undamaged material properties.  The amount of damage evolved is represented by the 
constant,  ω,  which  varies  from  zero  if  no  damage  has  occurred  to  unity  for  complete 
rupture.  For uniaxial loading, the nominal stress in the damaged material is given by  
where 𝑃 is the applied load and 𝐴 is the surface area.  The true stress is given by:  
𝜎nominal =
,
(22.79.2)
𝜎true =
𝐴 − 𝐴loss
,
(22.79.3)
where 𝐴loss is the void area.  The damage variable can then be defined:
Material Models 
LS-DYNA Theory Manual 
𝜔 =
𝐴loss
, 0 ≤ 𝜔 ≤ 1.
(22.79.4)
In this model damage is defined in terms of plastic strain after the failure strain is 
exceeded: 
𝜔 =
p − 𝜀failure
𝜀eff
− 𝜀failure
𝜀rupture
    if    𝜀failure
≤ 𝜀eff
p ≤ 𝜀rupture
. 
(22.79.5)
After exceeding the failure strain softening begins and continues until the rupture strain 
is reached.
LS-DYNA Theory Manual 
Material Models 
22.80  Material Model 101:  GE Thermoplastics 
The constitutive model for this approach is: 
𝜀̇p = 𝜀̇0exp(𝐴{𝜎 − 𝑆(𝜀p)}) × exp(−𝑝𝛼𝐴),
(22.80.1)
where  𝜀̇0  and  A  are  rate  dependent  yield  stress  parameters,  𝑆(𝜀𝑝)  internal  resistance 
(strain hardening) and 𝛼 is a pressure dependence parameter. 
In this material the yield stress may vary throughout the finite element model as 
a function of strain rate and hydrostatic stress.  Post yield stress behavior is captured in 
material softening and hardening values.  Finally, ductile or brittle failure measured by 
plastic  strain  or  maximum  principal  stress  respectively  is  accounted  for  by  automatic 
element deletion. 
Although  this  may  be  applied  to  a  variety  of  engineering  thermoplastics,  GE 
Plastics  have  constants  available  for  use  in  a  wide  range  of  commercially  available 
grades of their engineering thermoplastics.
Material Models 
LS-DYNA Theory Manual 
22.81  Material Model 102:  Hyperbolic Sine 
Resistance  to  deformation  is  both  temperature  and  strain  rate  dependent.    The 
flow stress equation is: 
𝜎 =
sinh−1
[
]
⎜⎜⎛
⎝
, 
⎟⎟⎞
⎠
where 𝑍, the Zener-Holloman temperature compensated strain rate, is: 
𝑍 = 𝜀̇exp (
𝐺𝑇
).
(22.81.1)
(22.81.2)
The  units  of  the  material  constitutive  constants  are  as  follows:  𝐴  (1/sec),  N 
(dimensionless), 𝛼 (1/MPa), the activation energy for flow, 𝑄 (J/mol), and the universal 
gas  constant,  𝐺  [J/(mol ⋅ K)].    The  value  of  𝐺  will  only  vary  with  the  unit  system 
chosen.  Typically it will be either 8.3145 J/(mol ⋅ K), or 40.8825 lb ⋅ in/mol ⋅ R. 
The  final  equation  necessary  to  complete  the  description  of  high  strain  rate 
deformation  herein  is  one  that  allows  computation  of  the  temperature  change  during 
the deformation.  In the absence of a coupled thermo-mechanical finite element code we 
assume adiabatic temperature change and follow the empirical assumption that 90-95% 
of the plastic work is dissipated as heat.  Thus the heat generation coefficient is 
HC ≈
0.9
𝜌𝐶𝑣
,
(22.81.3)
where 𝜌 is the material density and 𝐶𝑣 is the specific heat.
LS-DYNA Theory Manual 
Material Models 
22.82  Material Model 103:  Anisotropic Viscoplastic 
(22.82.1)
(22.82.2)
𝜎(𝜀eff
𝑝 , 𝜀̇eff
The uniaxial stress-strain curve is given on the following form 
𝑝 )]
𝑝 ) = 𝜎0 + 𝑄𝑟1[(1 − 𝑒𝑥𝑝(−𝐶𝑟1𝜀eff
𝑝 ))] + 𝑉𝑘𝜀̇eff
𝑝 ))] + 𝑄𝑟2[1 − 𝑒𝑥𝑝(−𝐶𝑟2𝜀eff
𝑝 ))] + 𝑄𝜒2[(1 − 𝑒𝑥𝑝(−𝐶𝜒2𝜀eff
+ 𝑄𝜒1[(1 − 𝑒𝑥𝑝(−𝐶𝜒1𝜀eff
𝑝 𝑉𝑚,
For bricks the following yield criteria is used 
𝐹(𝜎22 − 𝜎33)2 + 𝐺(𝜎33 − 𝜎11)2 + 𝐻(𝜎11 − 𝜎22)2 + 2𝐿𝜎23
𝑝 )]
𝑝 , 𝜀̇eff
𝑝   is  the  effective  plastic  strain  and  𝜀̇eff
= [𝜎(𝜀eff
,
𝑝   is  the  effective  plastic  strain  rate.    For 
where  𝜀eff
shells the anisotropic behavior is given by 𝑅00, 𝑅45 and 𝑅90.  When 𝑉𝑘 = 0 the material 
will behave elasto-plastically.  Default values are given by: 
2 + 2𝑀𝜎31
2 + 2𝑁𝜎12
𝐹 = 𝐺 = 𝐻 =
𝐿 = 𝑀 = 𝑁 =
,
,
𝑅00 = 𝑅45 = 𝑅90 = 1.
(22.82.3)
(22.82.4)
(22.82.5)
Strain rate is accounted for using the Cowper-Symonds model which, e.g., model 
3, scales the yield stress with the factor: 
1 + (
𝑝⁄
)
.
𝜀̇
(22.82.6)
To  convert  these  constants  set  the  viscoelastic  constants,  𝑉𝑘  and  𝑉𝑚,  to  the  following 
values: 
)
, 
(22.82.7)
𝑉𝑘 = 𝜎 (
𝑉𝑚 =
.
This  model  properly  treats  rate  effects  and  should  provide  superior  results  to 
models 3 and 24.
Material Models 
LS-DYNA Theory Manual 
22.83  Material Model 104:  Continuum Damage Mechanics 
Model 
Anisotropic  Damage  model  (FLAG = −1).  At  each  thickness  integration  points, 
an  anisotorpic  damage  law  acts  on  the  plane  stress  tensor  in  the  directions  of  the 
principal total shell strains, ε1 and 𝜀2, as follows: 
𝜎11 = (1 − 𝐷1(𝜀1))𝜎110,
𝜎22 = (1 − 𝐷2(𝜀2))𝜎220, 
𝜎12 = (1 −
𝐷1 + 𝐷2
) 𝜎120.
(22.83.1) 
The transverse plate shear stresses in the principal strain directions are assumed 
to be damaged as follows: 
𝜎13 = (1 −
𝜎23 = (1 −
𝐷1
𝐷2
) 𝜎130,
) 𝜎230.
(22.83.2) 
In  the  anisotropic  damage  formulation,  𝐷1(𝜀1)  and  𝐷2(𝜀2)  are  anisotropic 
damage  functions  for  the  loading  directions  1  and  2,  respectively.    Stresses  𝜎110,  𝜎220, 
 𝜎120, 𝜎130 and 𝜎230 are stresses in the principal shell strain directions as calculated from 
the  undamaged  elastic-plastic  material  behavior.    The  strains  𝜀1  and  𝜀2  are  the 
magnitude  of  the  principal  strains  calculated  upon  reaching  the  damage  thresholds.  
Damage  can  only  develop  for  tensile  stresses,  and  the  damage  functions  𝐷1(𝜀1)  and 
𝐷2(𝜀2) are identical to zero for negative strains 𝜀1 and 𝜀2. The principal strain directions 
are fixed within an integration point as soon as either principal strain exceeds the initial 
threshold  strain  in  tension.    A  more  detailed  description  of  the  damage  evolution  for 
this material model is given in the description of material 82. 
The Continuum Damage Mechanics (CDM) model (FLAG≥0) is based on a CDM 
model  proposed  by  Lemaitre  [1992].    The  effective  stress  𝜎̃ ,  which  is  the  stress 
calculated over the section that effectively resist the forces and reads. 
𝜎̃ =
1 − 𝐷
,
(22.83.3)
where  𝐷  is  the  damage  variable.    The  evolution  equation  for  the  damage  variable  is 
defined as
LS-DYNA Theory Manual 
Material Models 
𝐷̇ =
⎧
{{
⎨
{{
⎩
𝑆(1 − 𝐷)
𝑟 ̇
for 𝑟 > 𝑟𝐷 and 𝜎1 > 0
otherwise
. 
(22.83.4)
where  𝑟𝐷  is  the  damage  threshold,  𝑌  is  a  positive  material  constant,  𝑆  is  the  strain 
energy  release  rate,  and  𝜎1  is  the  maximal  principal  stress.    The  strain  energy  density 
release rate is  
𝑌 =
𝐞e: 𝐂: 𝐞e =
2 𝑅𝑣
𝜎vm
2𝐸(1 − 𝐷)2,
(22.83.5)
where 𝜎vm is the equivalent von Mises stress.  The triaxiality function 𝑅𝑣 is defined as  
𝑅𝑣 =
(1 + 𝜈) + 3(1 − 2𝜈) (
𝜎H
𝜎vm
)
.
The uniaxial stress-strain curve is given in the following form 
𝜎(𝑟, 𝜀̇eff
p ) = 𝜎0 + 𝑄1(1 − exp(−𝐶1𝑟)) + 𝑄2(1 − exp(−𝐶2𝑟)) + 𝑉𝑘𝜀̇eff
p 𝑉𝑚, 
where 𝑟 is the damage accumulated plastic strain, which can be calculated by 
𝑟 ̇ = 𝜀̇eff
p (1 − 𝐷).
For bricks the following yield criteria is used 
𝐹(𝜎̃22 − 𝜎̃33)2 + 𝐺(𝜎̃33 − 𝜎̃11)2 + 𝐻(𝜎̃11 − 𝜎̃22)2 + 2𝐿𝜎̃23
2 + 2𝑀𝜎̃31
2 + 2𝑁𝜎̃12
= 𝜎(𝑟, 𝜀̇eff
p ), 
(22.83.6)
(22.83.7)
(22.83.8)
(22.83.9)
p   is  the  effective  viscoplastic 
where  𝑟  is  the  damage  effective  viscoplastic  strain  and  𝜀̇eff
strain  rate.    For  shells  the  anisotropic  behavior  is  given  by  the  R-values:  𝑅00,  𝑅45,  and 
𝑅90.    When  𝑉𝑘 = 0  the  material  will  behave  as  an  elastoplastic  material  without  rate 
effects.  Default values for the anisotropic constants are given by: 
𝐹 = 𝐺 = 𝐻 =
𝐿 = 𝑀 = 𝑁 =
,
,
𝑅00 = 𝑅45 = 𝑅90 = 1,
(22.83.10)
(22.83.11)
(22.83.12)
so that isotropic behavior is obtained. 
Strain  rate  is  accounted  for  using the  Cowper-Symonds  model  which  scales  the 
yield stress with the factor:
Material Models 
LS-DYNA Theory Manual 
p⁄
)
.
1 + (
𝜀̇
(22.83.13)
To  convert  these  constants,  set  the  viscoelastic  constants,  𝑉𝑘  and  𝑉𝑚,  to  the 
following values: 
)
, 
(22.83.14)
𝑉𝑘 = 𝜎 (
𝑉𝑚 =
.
LS-DYNA Theory Manual 
Material Models 
22.84  Material Model 106:  Elastic Viscoplastic Thermal 
If LCSS is not given any value the uniaxial stress-strain curve has the form 
p ) = 𝜎0 + 𝑄𝑟1(1 − exp(−𝐶𝑟1𝜀eff
𝜎(𝜀eff
+𝑄χ1(1 − exp(−𝐶χ1𝜀eff
p )) + Qχ2(1 − exp(−Cχ2𝜀eff
p )).
p )) + 𝑄𝑟2(1 − exp(−𝐶𝑟2𝜀eff
p ))
(22.84.1)
Viscous  effects  are  accounted  for  using  the  Cowper-Symonds  model,  which 
scales the yield stress with the factor: 
1 + (
p⁄
)
.
𝜀̇eff
(22.84.2)
Material Models 
LS-DYNA Theory Manual 
22.85  Material Model 110:  Johnson-Holmquist Ceramic 
Model 
The  Johnson-Holmquist  plasticity  damage  model  is  useful  for  modeling 
ceramics, glass and other brittle materials.  A more detailed description can be found in 
a paper by Johnson and Holmquist [1993]. 
The equivalent stress for a ceramic-type material is given in terms of the damage 
parameter 𝐷 by 
Here, 
𝜎 ∗ = 𝜎i
∗ − 𝐷(𝜎i
∗ − 𝜎f
∗).
∗ = 𝑎(𝑝∗ + 𝑡∗)𝑛(1 + 𝑐ln𝜀̇∗),
𝜎i
(22.85.1)
(22.85.2)
represents the intact, undamaged behavior.   The superscript, '*', indicates a normalized 
quantity.    The  stresses  are  normalized  by  the  equivalent  stress  at  the  Hugoniot  elastic 
limit , the pressures are normalized by the pressure at the Hugoniot elastic 
limit,  and  the  strain  rate  by  the  reference  strain  rate  defined  in  the  input.    In  this 
equation  𝑎  is  the  intact normalized  strength  parameter, 𝑐  is  the  strength  parameter  for 
strain rate dependence, 𝜀̇∗ is the normalized plastic strain rate, and,  
𝑡∗ =
𝑝∗ =
PHEL
PHEL
,
,
(22.85.3) 
where 𝑇 is the maximum tensile pressure strength, PHEL is the pressure component at 
the Hugoniot elastic limit, and p is the pressure. 
p,
𝐷 = ∑ Δ𝜀p/𝜀f
(22.85.4)
represents  the  accumulated  damage  based  upon  the  increase  in  plastic  strain  per 
computational cycle and the plastic strain to fracture 
p = 𝑑1(𝑝∗ + 𝑡∗)𝑑2,
𝜀f
where 𝑑1 and 𝑑2 are user defined input parameters.  The equation: 
∗ = 𝑏(𝑝∗)𝑚(1 + 𝑐ln𝜀̇∗) ≤ SFMAX,
𝜎f
(22.85.5)
(22.85.6)
represents  the  damaged  behavior  where  𝑏  is  an  input  parameter  and  SFMAX  is  the 
maximum normalized fracture strength.  The parameter, 𝑑1, controls the rate at which 
damage  accumulates.    If  it  approaches  0,  full  damage  can  occur  in  one  time  step,  i.e., 
instantaneously.  This rate parameter is also the best parameter to vary if one attempts 
to reproduce results generated by another finite element program.
LS-DYNA Theory Manual 
Material Models 
In undamaged material, the hydrostatic pressure is given by 
𝑝 = 𝑘1𝜇 + 𝑘2𝜇2 + 𝑘3𝜇3,
(22.85.7)
where 𝜇 = 𝜌/𝜌0 − 1.  When damage starts to occur, there is an increase in pressure.  A 
fraction defined in the input, between 0 and 1, of the elastic energy loss, 𝛽, is converted 
into hydrostatic potential energy, which results in an increase in pressure.  The details 
of this pressure increase are given in the reference. 
Given HEL and the shear modulus, 𝑔, 𝜇hel can be found iteratively from 
HEL = 𝑘1𝜇hel + 𝑘2𝜇hel
2 + 𝑘3𝜇hel
3 +
𝑔 (
𝜇hel
1 + 𝜇hel
),
and, subsequently, for normalization purposes, 
and 
PHEL = 𝑘1𝜇hel + 𝑘2𝜇hel
2 + 𝑘3𝜇hel
3 ,
𝜎hel = 1.5(HEL − PHEL).
These are calculated automatically by LS-DYNA if PHEL is zero on input.
(22.85.8)
(22.85.9)
(22.85.10)
Material Models 
LS-DYNA Theory Manual 
22.86  Material Model 111:  Johnson-Holmquist Concrete 
Model  
This model can be used for concrete subjected to large strains, high strain rates, 
and high pressures.  The equivalent strength is expressed as a function of the pressure, 
strain  rate,  and  damage.    The  pressure  is  expressed  as  a  function  of  the  volumetric 
strain and includes the effect of permanent crushing.  The damage is accumulated as a 
function of the plastic volumetric strain, equivalent plastic strain and pressure.  A more 
detailed  description  of  this  model  can  be  found  in  the  paper  by  Holmquist,  Johnson, 
and Cook [1993] 
The normalized equivalent stress is defined as 
𝜎 ∗ =
′,
𝑓c
(22.86.1)
where  𝜎  is  the  actual  equivalent  stress,  and  𝑓c
strength.  The yield stress is defined in terms of the input parameters 𝑎, 𝑏, 𝑐, and 𝑛 as: 
′  is  the  quasi-static  uniaxial  compressive 
𝜎 ∗ = [𝑎(1 − 𝐷) + 𝑏𝑝∗𝑛][1 − 𝑐ln(𝜀̇∗)],
(22.86.2)
′ is the normalized pressure and 𝜀̇∗ = 𝜀̇/𝜀̇0 is 
where 𝐷 is the damage parameter, 𝑝∗ = 𝑝/𝑓c
the  dimensionless  strain  rate.    The  model  accumulates  damage  both  from  equivalent 
plastic strain and plastic volumetric strain, and is expressed as 
𝐷 = ∑
Δ𝜀p + Δ𝜇p
𝐷1(𝑝∗ + 𝑇∗)𝐷2
where  Δ𝜀p  and  Δ𝜇p  are  the  equivalent  plastic  strain  and  plastic  volumetric  strain,  𝐷1 
′  is  the  normalized  maximum  tensile 
and  𝐷2  are  material  constants  and  𝑇∗ = 𝑇/𝑓c
hydrostatic pressure where 𝑇 is the maximum tensile hydrostatic pressure. 
(22.86.3)
,
The pressure for fully dense material is expressed as: 
𝑃 = 𝐾1𝜇̅̅̅̅ + 𝐾2𝜇̅̅̅̅2 + 𝐾3𝜇̅̅̅̅3,
(22.86.4)
where  𝐾1  ,  𝐾2  and  𝐾3  are  material  constants  and  the  modified  volumetric  strain  is 
defined as 
𝜇̅̅̅̅ =
𝜇 − 𝜇lock
1 + 𝜇lock
,
(22.86.5)
where 𝜇lock is the locking volumetric strain.
LS-DYNA Theory Manual 
Material Models 
22.87  Material Model 115:  Elastic Creep Model 
The effective creep strain, 𝜀̅c, given as: 
𝜀̅c = 𝐴𝜎̅̅̅̅̅ 𝑛𝑡 ̅𝑚,
(22.87.1)
where  𝐴,  𝑛,  and  𝑚  are  constants  and  𝑡 ̅  is  the  effective  time.    The  effective  stress,  𝜎̅̅̅̅̅,  is 
defined as: 
𝜎̅̅̅̅̅ = √
𝜎𝑖𝑗𝜎𝑖𝑗.
(22.87.2)
The  creep  strain,  therefore,  is  only  a  function  of  the  deviatoric  stresses.    The 
volumetric  behavior  for  this  material  is  assumed  to  be  elastic.    By  varying  the  time 
constant  𝑚  primary  creep  (𝑚 < 1),  secondary  creep  (𝑚 = 1),  and  tertiary  creep  (𝑚 > 1) 
can be modeled.  This model is described by Whirley and Henshall (1992).
Material Models 
LS-DYNA Theory Manual 
22.88  Material Model 116:  Composite Layup  
This material is for modeling the elastic responses of composite lay-ups that have 
an arbitrary number of layers through the shell thickness.  A pre-integration is used to 
compute  the  extensional,  bending,  and  coupling  stiffness  for  use  with  the  Belytschko-
Tsay  resultant  shell  formulation.    The  angles  of  the  local  material  axes  are  specified 
from layer to layer in the *SECTION_SHELL input.  This material model must be used 
with  the  user  defined  integration  rule  for  shells,  which  allows  the  elastic  constants  to 
change from integration point to integration point.  Since the stresses are not computed 
in the resultant formulation, the stress output to the binary databases for the resultant 
elements are zero. 
  The 
This  material  law  is  based  on  standard  composite  lay-up  theory. 
implementation,  [Jones  1975],  allows  the  calculation  of  the  force,  𝐍,  and  moment,  𝐌, 
stress resultants from:  
⎧𝑁𝑥
⎫
}
{
𝑁𝑦
⎬
⎨
}
{
𝑁𝑥𝑦⎭
⎩
=
𝐴11 𝐴12 𝐴16
⎤
⎡
𝐴21 𝐴22 𝐴26
⎥
⎢
𝐴16 𝐴26 𝐴66⎦
⎣
⎫
⎧𝜀𝑥
}}
{{
𝜀𝑦
⎬
⎨
}}
{{
0⎭
𝜀𝑧
⎩
+
𝐵11 𝐵12
𝐵16
⎤
𝐵21 𝐵22 𝐵26
⎥
𝐵16 𝐵26 𝐵66⎦
⎡
⎢
⎣
{⎧ 𝜅𝑥
}⎫
𝜅𝑦
𝜅𝑥𝑦⎭}⎬
⎩{⎨
, 
⎧𝑀𝑥
⎫
}
{
𝑀𝑦
⎬
⎨
}
{
𝑀𝑥𝑦⎭
⎩
=
𝐵11 𝐵12 𝐵16
⎤
⎡
𝐵21 𝐵22 𝐵26
⎥
⎢
𝐵16 𝐵26 𝐵66⎦
⎣
⎫
⎧𝜀𝑥
}}
{{
𝜀𝑦
⎬
⎨
}}
{{
0⎭
𝜀𝑧
⎩
+
𝐷11 𝐷12 𝐷16
⎤
⎡
𝐷21 𝐷22 𝐷26
⎥
⎢
𝐷16 𝐷26 𝐷66⎦
⎣
{⎧ 𝜅𝑥
}⎫
𝜅𝑦
𝜅𝑥𝑦⎭}⎬
⎩{⎨
, 
(22.88.1)
(22.88.2)
where 𝐴𝑖𝑗 is the extensional stiffness, 𝐷𝑖𝑗 is the bending stiffness, and 𝐵𝑖𝑗 is the coupling 
stiffness,  which  is  a  null  matrix  for  symmetric  lay-ups.    The  mid-surface  strains  and 
0   and  𝜅𝑖𝑗,  respectively.    Since  these  stiffness  matrices  are 
curvatures  are  denoted  by  𝜀𝑖𝑗
symmetric,  18  terms  are  needed  per  shell  element  in  addition  to  the  shell  resultants, 
which are integrated in time.  This is considerably less storage than would typically be 
required with through thickness integration which requires a minimum of eight history 
variables  per  integration  point,  e.g.,  if  100  layers  are  used  800  history  variables  would 
be stored.  Not only is memory much less for this model, but the CPU time required is 
also considerably reduced.
LS-DYNA Theory Manual 
Material Models 
22.89  Material Model 117-118:  Composite Matrix  
This material is used for modeling the elastic responses of composites where pre-
integration, which is done outside of LS-DYNA unlike the lay-up option above, is used 
to compute the extensional, bending, and coupling stiffness coefficients for use with the 
Belytschko-Tsay and the assumed strain resultant shell formulations.  Since the stresses 
are  not  computed  in  the  resultant  formulation,  the  stresses  output  to  the  binary 
databases for the resultant elements are zero. 
⎫
The  calculation  of  the  force,  𝑁𝑖𝑗,  and  moment,  𝑀𝑖𝑗,  stress  resultants  is  given  in 
0, and shell curvatures, 𝜅𝑖, as:  
⎧ 𝜀𝑥
𝜀𝑦
𝜀𝑧
𝜅𝑥
𝜅𝑦
𝜅𝑥𝑦⎭
𝐶11 𝐶12 𝐶13 𝐶14 𝐶15 𝐶16
⎤
⎡
𝐶21 𝐶22 𝐶23 𝐶24 𝐶25 𝐶26
⎥
⎢
⎥
⎢
𝐶31 𝐶32 𝐶33 𝐶34 𝐶35 𝐶36
⎥
⎢
⎥
⎢
𝐶41 𝐶42 𝐶43 𝐶44 𝐶45 𝐶46
⎥
⎢
𝐶51 𝐶52 𝐶53 𝐶54 𝐶55 𝐶56
⎥
⎢
𝐶61 𝐶62 𝐶63 𝐶64 𝐶65 𝐶66⎦
⎣
terms of the membrane strains, 𝜀𝑖
⎧ 𝑁𝑥
𝑁𝑦
𝑁𝑥𝑦
𝑀𝑥
𝑀𝑦
𝑀𝑥𝑦⎭
}}}}}
}}}}}
{{{{{
{{{{{
}}}}}
}}}}}
{{{{{
{{{{{
(22.89.1)
=
, 
⎫
⎬
⎩
⎨
⎨
⎩
⎬
where  𝐶𝑖𝑗 = 𝐶𝑗𝑖.    In  this  model  this  symmetric  matrix  is  transformed  into  the  element 
local system and the coefficients are stored as element history variables.   
In  a  variation  of  this  model,  *MAT_COMPOSITE_DIRECT,  the  resultants  are 
already  assumed  to  be  given  in  the  element  local  system  which  reduces  the  storage 
since the 21 coefficients are not stored as history variables as part of the element data.  
The shell thickness is built into the coefficient matrix and, consequently, within the part 
ID, which references this material ID, the thickness must be uniform.
Material Models 
LS-DYNA Theory Manual 
22.90  Material Model 119:  General Nonlinear 6DOF Discrete 
Beam 
Catastrophic  failure,  which  is  based  on  displacement  resultants,  occurs  if  either 
of the following inequalities are satisfied: 
(
𝑢r
tfail
𝑢r
)
+ (
)
𝑢s
tfail
𝑢s
+ (
𝑢t
tfail
𝑢t
)
+ (
𝜃r
tfail
𝜃r
)
+ (
𝜃s
tfail
𝜃s
)
+ (
𝜃t
tfail
𝜃t
)
− 1. ≥ 0, 
(22.90.1) 
(
𝑢r
cfail
𝑢r
)
+ (
𝑢s
cfail
𝑢s
)
+ (
𝑢t
cfail
𝑢t
)
+ (
𝜃r
cfail
𝜃r
)
+ (
𝜃s
cfail
𝜃s
)
+ (
𝜃t
cfail
𝜃t
)
− 1. ≥ 0. 
(22.90.2) 
After  failure  the  discrete  element  is  deleted.    If  failure  is  included  either  the 
tension failure or the compression failure or both may be used.
Unload = 0
loading-unloading 
curve
Unload = 2
Unloading curve
Unloading curve
Unload = 1
Displacement
Displacement
Unload = 3
Unloading curve
Displacement
Displacement
Figure 22.90.1.  Load and unloading behavior. 
Umin
OFFSET x Umin
LS-DYNA Theory Manual 
Material Models 
22.91  Material Model 120:  Gurson 
The Gurson flow function is defined as: 
𝛷 =
𝜎M
2 + 2𝑞1𝑓 ∗cosh (
𝜎Y
3𝑞2𝜎H
2𝜎Y
) − 1 − (𝑞1𝑓 ∗)2 = 0,
(22.91.1)
where  𝜎M  is  the  equivalent  von  Mises  stress,  𝜎Y  is  the  Yield  stress,  𝜎H  is  the  mean 
hydrostatic stress.  The effective void volume fraction is defined as 
𝑓 ∗(𝑓 ) =
⎧
{{{
⎨
{{{
⎩
𝑓 ≤ 𝑓c
. 
𝑓c +
1/𝑞1 − 𝑓c
𝑓F − 𝑓c
(𝑓 − 𝑓c)
𝑓 > 𝑓c
The growth of void volume fraction is defined as 
𝑓 ̇ = 𝑓 ̇
G + 𝑓 ̇
N,
where the growth of existing voids is defined as 
p ,
𝑓 ̇
G = (1 − 𝑓 )𝜀̇𝑘𝑘
and the nucleation of new voids is defined as 
𝑓 ̇
N = 𝐴𝜀̇p,
where  
𝐴 =
𝑓N
𝑆N√2π
exp (−
(
𝜀p − 𝜀N
𝑆N
)
).
(22.91.2)
(22.91.3)
(22.91.4)
(22.91.5)
(22.91.6)
Material Models 
LS-DYNA Theory Manual 
22.92  Material Model 120:  Gurson RCDC 
The Rc-Dc model is defined as follows.  The damage 𝐷 is given by 
where 𝜀p is the equivalent plastic strain,  
𝐷 = ∫ 𝜔1𝜔2𝑑𝜀p,
𝜔1 = (
1 − 𝛾𝜎m
)
,
(22.92.1)
(22.92.2)
is the triaxial stress weighting term and 
𝜔2 = (2 − 𝐴D)𝛽,
is the asymmetric strain weighting term.  In the above 𝜎m is the mean stress and  
(22.92.3)
𝐴D = min (∣
𝑆2
𝑆3
∣ , ∣
𝑆3
𝑆2
∣).
Fracture is initiated when the accumulation of damage satisfies 
𝐷c
> 1,
where 𝐷c is the critical damage given by 
𝐷c = 𝐷0(1 + 𝑏|∇𝐷|λ).
(22.92.4)
(22.92.5)
(22.92.6)
LS-DYNA Theory Manual 
Material Models 
22.93  Material Model 124:  Tension-Compression Plasticity 
This  is  an  isotropic  elastic-plastic  material  where  a  unique  yield  stress  versus 
plastic  strain  curve  can  be  defined  for  compression  and  tension.    Failure  can  occur 
based on plastic strain or a minimum time step size.  Rate effects are modeled by using 
the Cowper-Symonds strain rate model. 
The  stress-strain  behavior  follows  one  curve  in  compression  and  another  in 
tension.  The sign of the mean stress determines the state where a positive mean stress 
(i.e., a negative pressure) is indicative of tension.  Two load curves, 𝑓t(𝑝) and 𝑓c(𝑝), are 
defined,  which  give  the  yield  stress,  𝜎y,  versus  effective  plastic  strain  for  both  the 
tension and compression regimes.  The two pressure values, 𝑝t and 𝑝c, when exceeded, 
determine if the tension curve or the compressive curve is followed, respectively.  If the 
pressure,  𝑝,  falls  between  these  two  values,  a  weighted  average  of  the  two  curves  are 
used: 
if    − 𝑝t ≤ 𝑝 ≤ 𝑝c     
{⎧scale =
⎩{⎨
𝑝c − 𝑝
𝑝c + 𝑝t
. 
(22.93.1)
𝜎y = scale ⋅ 𝑓t(𝑝) + (1 − scale) ⋅ 𝑓c(𝑝)
Strain rate is accounted for using the Cowper and Symonds model, which scales 
the yield stress with the factor 
p⁄
)
,
1 + (
𝜀̇
(22.93.2)
where 𝜀̇ is the strain rate 𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗.
Material Models 
LS-DYNA Theory Manual 
22.94  Material Model 126:  Metallic Honeycomb 
For  efficiency  it  is  strongly  recommended  that  the  load  curve  ID’s:  LCA,  LCB, 
LCC,  LCS,  LCAB,  LCBC,  and  LCCA,  contain  exactly  the  same  number  of  points  with 
corresponding  strain  values  on  the  abscissa.    If  this  recommendation  is  followed  the 
cost  of  the  table  lookup  is  insignificant.    Conversely,  the  cost  increases  significantly  if 
the abscissa strain values are not consistent between load curves.  
The  behavior  before  compaction  is  orthotropic  where  the  components  of  the 
stress  tensor  are  uncoupled,  i.e.,  a  component  of  strain  will  generate  resistance  in  the 
local a-  direction  with  no  coupling  to  the  local  𝑏  and  𝑐  directions.    The  elastic  modulii 
vary  from  their  initial  values  to  the  fully  compacted  values  linearly  with  the  relative 
volume: 
𝐸𝑎𝑎 = 𝐸𝑎𝑎𝑢 + 𝛽𝑎𝑎(𝐸 − 𝐸𝑎𝑎𝑢), 𝐺𝑎𝑏 = 𝐺𝑎𝑏𝑢 + 𝛽(𝐺 − 𝐺𝑎𝑏𝑢),
𝐸𝑏𝑏 = 𝐸𝑏𝑏𝑢 + 𝛽𝑏𝑏(𝐸 − 𝐸𝑏𝑏𝑢), 𝐺𝑏𝑐 = 𝐺𝑏𝑐𝑢 + 𝛽(𝐺 − 𝐺𝑏𝑐𝑢),
𝐸𝑐𝑐 = 𝐸𝑐𝑐𝑢 + 𝛽𝑐𝑐(𝐸 − 𝐸𝑐𝑐𝑢), 𝐺𝑐𝑎 = 𝐺𝑐𝑎𝑢 + 𝛽(𝐺 − 𝐺𝑐𝑎𝑢),
where  
𝛽 = max [min (
1 − 𝑉
1 − 𝑉𝑓
, 1) , 0],
and 𝐺 is the elastic shear modulus for the fully compacted honeycomb material 
𝐺 =
2(1 + 𝜈)
.
(22.94.1)
(22.94.2)
(22.94.3)
The  relative  volume,  𝜈,  is  defined  as  the  ratio  of  the  current  volume  over  the 
initial volume, and typically, 𝜈 = 1 at the beginning of a calculation.  
The  load  curves  define  the  magnitude  of  the  stress  as  the  material  undergoes 
deformation.    The  first  value  in  the  curve  should  be  less  than  or  equal  to  zero 
corresponding to tension and increase to full compaction.  Care should be taken when 
defining the curves so the extrapolated values do not lead to negative yield stresses. 
At  the  beginning  of the  stress  update  we  transform  each  element’s  stresses  and 
strain rates into the local element coordinate system.  For the uncompacted material, the 
trial stress components are updated using the elastic interpolated modulii according to: 
𝑛+1trial
𝑛+1trial
𝑛+1trial
𝜎𝑎𝑎
𝜎𝑏𝑏
𝜎𝑐𝑐
= 𝜎𝑎𝑎
= 𝜎𝑏𝑏
= 𝜎𝑐𝑐
𝑛 + 𝐸𝑎𝑎Δ𝜀𝑎𝑎, 𝜎𝑎𝑏
𝑛 + 𝐸𝑏𝑏Δ𝜀𝑏𝑏, 𝜎𝑏𝑐
𝑛 + 𝐸𝑐𝑐Δ𝜀𝑐𝑐,
𝜎𝑐𝑎
𝑛+1trial
𝑛+1trial
𝑛+1trial
= 𝜎𝑎𝑏
= 𝜎𝑏𝑐
= 𝜎𝑐𝑎
𝑛 + 2𝐺𝑎𝑏Δ𝜀𝑎𝑏,
𝑛 + 2𝐺𝑏𝑐Δ𝜀𝑏𝑐,
𝑛 + 2𝐺𝑐𝑎Δ𝜀𝑐𝑎,
(22.94.4)
LS-DYNA Theory Manual 
Material Models 
We then independently check each component of the updated stresses to ensure 
that they do not exceed the permissible values determined from the load curves, e.g., if 
then 
𝑛+1trial
∣𝜎𝑖𝑗
∣ > 𝜆𝜎𝑖𝑗(𝜀𝑖𝑗),
𝑛+1 = 𝜎𝑖𝑗(𝜀𝑖𝑗)
𝜎𝑖𝑗
𝑛+1trial
𝜆𝜎𝑖𝑗
𝑛+1trial∣
∣𝜎𝑖𝑗
. 
(22.94.5)
(22.94.6)
The components of 𝜎𝑖𝑗(𝜀𝑖𝑗) are defined by load curves.  The parameter 𝜆 is either 
unity or a value taken from the load curve number, LCSR, that defines 𝜆 as a function of 
strain-rate.    Strain-rate  is  defined  here  as  the  Euclidean  norm  of  the  deviatoric  strain-
rate tensor. 
For  fully  compacted  material  we  assume  that  the  material  behavior  is  elastic-
perfectly plastic and updated the stress components according to: 
trial = 𝑠𝑖𝑗
𝑠𝑖𝑗
𝑛 + 2𝐺Δ𝜀𝑖𝑗
dev𝑛+1
2⁄
,
where the deviatoric strain increment is defined as 
Δ𝜀𝑖𝑗
dev = Δ𝜀𝑖𝑗 −
Δ𝜀𝑘𝑘𝛿𝑖𝑗.
(22.94.7)
(22.94.8)
We  now  check  to  see  if  the  yield  stress  for  the  fully  compacted  material  is 
exceeded by comparing 
trial = (
𝑠eff
2⁄
trial)
trial𝑠𝑖𝑗
𝑠𝑖𝑗
,
(22.94.9)
the  effective  trial  stress  to  the  yield  stress,  σy.    If  the  effective  trial  stress  exceeds  the 
yield stress, we simply scale back the stress components to the yield surface 
𝑛+1 =
𝑠𝑖𝑗
𝜎y
trial
𝑠eff
trial.
𝑠𝑖𝑗
We can now update the pressure using the elastic bulk modulus, K 
2⁄
𝑛+1
𝑝𝑛+1 = 𝑝𝑛 − 𝐾Δ𝜀𝑘𝑘
,
3(1 − 2𝜈)
𝐾 =
,
and obtain the final value for the Cauchy stress 
𝑛+1 = 𝑠𝑖𝑗
𝜎𝑖𝑗
𝑛+1 − 𝑝𝑛+1𝛿𝑖𝑗.
(22.94.10)
(22.94.11)
(22.94.12)
Material Models 
LS-DYNA Theory Manual 
After  completing  the  stress  update  we  transform  the  stresses  back  to  the  global 
configuration. 
22.94.1  Stress Update 
If LCA < 0, a transversely anisotropic yield surface is obtained where the uniaxial 
limit stress, 𝜎 y(𝜑, 𝜀vol), can be defined as a function of angle 𝜑 with the strong axis and 
volumetric strain, 𝜀vol.  Elastically, the new material model is assumed to behave exactly 
as  material  126  (with  the  restriction  𝐸22𝑢 = 𝐸33𝑢  and  𝐺12𝑢 = 𝐺13𝑢),  see  the  LS-DYNA 
Keyword  User’s  Manual  [Hallquist  2003].    As  for  the  plastic  behavior,  a  natural 
question that arises is how to define the limit stress for a general multiaxial stress state 
that reduces to the uniaxial limit stress requirement when the stress is uniaxial.  Having 
given  it  some  thought,  we  feel  that  it  is  most  convenient  to  work  with  the  principal 
stresses and the corresponding directions to achieve this goal. 
Assume  that  the  elastic  update  results  in  a  trial  stress  𝜎 trial  in  the  material 
coordinate  system.    This  stress  tensor  is  diagonalized  to  obtain  the  principal  stresses 
trial and the corresponding principal directions 𝐪1, 𝐪2 and 𝐪3 relative to 
trial, 𝜎2
𝜎1
the  material  coordinate  system.    The  angle  that  each  direction  makes  with  the  strong 
axis of anisotropy 𝐞1 is given by  
trial and 𝜎3
Curve extends into negative strain 
quadrant since LS-DYNA will 
extrapolate using the two end points.
It is important that the extropolation 
does not extend into the negative stress 
region.
 σij
unloading and
reloading path
Strain: -εij
Unloading is based on the interpolated Young’s 
moduli which must provide an unloading 
tangent that exceeds the loading tangent.
Figure 22.94.1.  Stress quantity versus strain.  Note that the “yield stress” at a 
strain of zero  is nonzero.  In the load curve definition  the “time” value is  the 
directional strain and the “function” value is the yield stress.
LS-DYNA Theory Manual 
Material Models 
𝜑𝑖 = arccos∣𝐪𝑖 ⋅ 𝐞1∣, 𝑖 = 1, 2, 3. 
(22.94.13)
Now a limit stress in the direction of a general multiaxial stress is determined as 
a convex combination of the uniaxial limit stress in each principal direction 
𝜎 Y(𝜎 trial) =
𝑗=1
∑ 𝜎 Y(𝜙j, 𝜀vol)𝜎𝑗
trial𝜎𝑘
∑ 𝜎𝑘
𝑘=1
trial𝜎𝑗
trial
trial
, 
(22.94.14)
Each of the principal stresses is updated as 
𝜎𝑖 = 𝜎𝑖
trialmin
1,
⎜⎜⎜⎜⎜⎛
⎝
𝜎 Y(𝜎 trial)
√∑ 𝜎𝑘
𝑘=1
trial𝜎𝑘
trial
, 
⎟⎟⎟⎟⎟⎞
⎠
(22.94.15)
and the new stress is transformed back to the material coordinate system3.  
This  stress  update  is  not  uniquely  defined  when  the  stress  tensor  possesses 
multiple eigenvalues,  thus the following simple set of rules is applied.  If all principal 
stresses are equal, one of the principal directions is chosen to coincide with the strong 
axis  of  anisotropy.    If  two  principal  stresses  are  equal,  then  one  of  the  directions 
corresponding  to  this  stress  value  is  chosen  perpendicular  to  the  strong  axis  of 
anisotropy. 
22.94.2  Support for Independent Shear and Hydrostatic Yield Stress Limit 
The model just described turned out to be weak in shear [Okuda 2003] and there 
were  no  means  of  adding  shear  resistance  without  changing  the  behavior  in  pure 
uniaxial compression.  We propose the following modification of the model where the 
user can prescribe the shear and hydrostatic resistance in the material without changing 
the uniaxial behavior. 
Assume  that  the  elastic  update  results  in  a  trial  stress  𝜎 trial  in  the  material 
coordinate  system.    This  stress  tensor  is  diagonalized  to  obtain  the  principal  stresses 
trial and the corresponding principal directions 𝐪1, 𝐪2 and 𝐪3 relative to 
trial, 𝜎2
𝜎1
the material coordinate system.  For this discussion we assume that the principal stress 
values are ordered so that 𝜎1
trial. Two cases need to be treated.  
trial and 𝜎3
trial ≤ 𝜎2
trial ≤ 𝜎3
3 Since each component of the stress tensor is scaled by the same factor in Equation 19.126.14, the stress is 
in  practice  not  transformed  back  but  the  scaling  is  performed  on  the  stress  in  the  material  coordinate 
system.
Material Models 
LS-DYNA Theory Manual 
trial ≤ −𝜎3
If  𝜎1
and consequently 𝜎1
trial  then  the  principal  stress  value  with  largest  magnitude  is  𝜎1
trial ≤ 0. Let  
trial, 
𝜎𝑢 = 𝜎1
𝜎p =
trial + max(∣𝜎2
trial∣, ∣𝜎3
trial∣),
{−max(∣𝜎2
trial∣, ∣𝜎3
trial∣) + 𝜎2
trial + 𝜎3
trial},
and finally 
trial∣, ∣𝜎3
trial∣) − 𝜎p 
1 = − max(∣𝜎2
𝜎d
2 = 𝜎2
trial − 𝜎p, 
𝜎d
3 = 𝜎3
trial − 𝜎p.
𝜎d
(22.94.16)
(22.94.17)
The  total  stress  is  the  sum  of  a  uniaxial  stress  represented  by  𝜎u,  a  hydrostatic 
3. The angle 
stress represented by 𝜎p and a deviatoric stress represented by 𝜎d
that  the  direction  of  𝜎u  makes  with  the  strong  axis  of  anisotropy  𝐞1  is  given  by  𝜙 =
arccos∣𝐪1 ⋅ 𝐞1∣. 
2 and 𝜎d
1, 𝜎d
Now  a  limit  stress  for  the  general  multiaxial  stress  is  determined  as  a  convex 
combination of the three stress contributions as follows 
𝜎 Y(𝜎 trial)
Y(𝜙, 𝜀vol)𝜎u
𝜎u
2 + 3√3𝜎p
Y(𝜀vol)𝜎p
2 + √2𝜎d
=
𝜎u
2 + 3𝜎p
2 + (𝜎d
1)2 + (𝜎d
1)2 + (𝜎d
Y(𝜀vol){(𝜎d
2)2 + (𝜎d
3)2
2)2 + (𝜎d
3)2}
(22.94.18)
. 
Y(𝜙, εvol) is the prescribed uniaxial stress limit, 𝜎p
Here 𝜎u
limit and 𝜎d
exactly as for the old model.  The other two functions are for now written 
Y(𝜀vol) is the hydrostatic stress 
Y(𝜀vol) is the stress limit in simple shear.  The input for the first of these is 
Y(𝜀vol) = 𝜎p
𝜎p
Y(𝜀vol) = 𝜎d
𝜎d
Y + 𝜎 S(𝜀vol),
Y + 𝜎 S(𝜀vol),
(22.94.19)
Y  and  𝜎d
Y  are  user  prescribed  constant  stress  limits  and  𝜎 S  is  the  function 
where  𝜎p
describing  the  densification  of  the  material when  loaded  in  the  direction  of  the  strong 
material axis.  We use the keyword parameters ECCU and GCAU for the new input as 
follows. 
•  ECCU σd
Y, average stress limit (yield) in simple shear. 
•  GCAU σp
Y, average stress limit (yield) in hydrostatic compression (pressure). 
Both of these parameters should be positive. 
Each of the principal stresses is updated as
LS-DYNA Theory Manual 
Material Models 
𝜎𝑖 = 𝜎𝑖
trialmin
1,
⎜⎜⎜⎜⎜⎛
⎝
𝜎 Y(𝜎 trial)
√∑ 𝜎𝑘
𝑘=1
trial𝜎𝑘
trial
, 
⎟⎟⎟⎟⎟⎞
⎠
(22.94.20)
and the new stress is transformed back to the material coordinate system.  
trial ≥ −σ1
If  σ3
and consequently σ3
trial  then  the  principal  stress  value  with  largest  magnitude  is  σ3
trial ≥ 0.  Let  
trial 
𝜎u = 𝜎3
𝜎p =
trial − max(∣𝜎2
trial∣, ∣𝜎1
trial∣),
{max(∣𝜎2
trial∣, ∣𝜎1
trial∣) + 𝜎2
trial + 𝜎1
trial}, 
and finally 
trial − 𝜎p,
trial − 𝜎p, 
1 = 𝜎1
𝜎d
2 = 𝜎2
𝜎d
3 = max(∣𝜎2
𝜎d
trial∣, ∣𝜎1
trial∣) − 𝜎p.
(22.94.21)
(22.94.22)
The angle that the direction of 𝜎u makes with the strong axis of anisotropy 𝐞1 is 
given by 𝜙 = arccos∣𝐪3 ⋅ 𝐞1∣.  The rest of the treatment is the same as for the case when 
trial.  To motivate the model, let us consider three states of stress. 
trial ≤ −𝜎3
𝜎1
1. 
2. 
3. 
For a uniaxial stress 𝜎, we have 𝜎u = 𝜎 and 𝜎p = 𝜎d
us  to  𝜎 Y(𝜎 trial) = 𝜎u
user prescribed uniaxial stress limit. 
3 = 0. This leads 
Y(𝜙, 𝜀vol)  and  hence  the  stress  level  will  be  limited  by  the 
2 = 𝜎d
1 = 𝜎d
For  a  simple  shear  𝜎,  we  have  𝜎d
𝜎 Y(𝜎 trial) = √2𝜎d
scribed shear stress limit. 
2 = 𝜎u = 0.  Hence 
Y(𝜀vol)  and  the  stress  level  will  be  limited  by  the  user  pre-
3 = −𝜎  and  𝜎p = 𝜎d
1 = −𝜎d
For  a  pressure  𝜎,  we  have  𝜎p = 𝜎  and  𝜎u = 𝜎d
3 = 0.  Hence 
Y(𝜀vol)  and  the  stress  level  will  be  limited  by  the  user  pre-
2 = 𝜎d
1 = 𝜎d
𝜎 Y(𝜎 trial) = √3𝜎p
scribed hydrostatic stress limit.
Material Models 
LS-DYNA Theory Manual 
22.95  Material Model 127:  Arruda-Boyce Hyperviscoelastic 
Rubber 
This  material  model,  described  in  the  paper  by  Arruda  and  Boyce  [1993], 
provides a rubber model that is optionally combined with linear viscoelasticity.  Rubber 
is  generally  considered  to  be  fully  incompressible  since  the  bulk  modulus  greatly 
exceeds  the  shear  modulus  in  magnitude;  therefore,  to  model  the  rubber  as  an 
unconstrained  material,  a  hydrostatic  work  term,  𝑊H(𝐽),  is  included  in  the  strain 
energy functional which is a function of the relative volume, 𝐽, [Ogden, 1984]: 
𝑊(𝐽1, 𝐽2, 𝐽) = 𝑛𝑘𝜃 [
(𝐽1 − 3) +
19
7000𝑁3 (𝐽1
(𝐽1
20𝑁
4 − 81) +
2 − 9) +
11
1050𝑁2 (𝐽1
519
673750𝑁4 (𝐽1
3 − 27)]
5 − 243)] + 𝑊H(𝐽), 
(22.95.1)
+ 𝑛𝑘𝜃 [
𝐽1 = 𝐼1𝐽−1
𝐽2 = 𝐼2𝐽. 
3⁄ , 
The hydrostatic work term is expressed in terms of the bulk modulus, 𝐾, and 𝐽, as: 
𝑊H(𝐽) =
(𝐽 − 1)2.
(22.95.2)
Rate  effects  are  taken  into  account  through  linear  viscoelasticity  by  a  convolution 
integral of the form: 
𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙
(𝑡 − 𝜏)
𝜕𝜀𝑘𝑙
𝜕𝜏
𝑑𝜏,
(22.95.3)
or in terms of the second Piola-Kirchhoff stress, 𝑆𝑖𝑗, and Green's strain tensor, 𝐸𝑖𝑗, 
𝑆𝑖𝑗 = ∫ 𝐺𝑖𝑗𝑘𝑙
(𝑡 − 𝜏)
𝜕𝐸𝑘𝑙
𝜕𝜏
𝑑𝜏,
(22.95.4)
where  𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)  and  𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏)  are  the  relaxation  functions  for  the  different  stress 
measures.    This  stress  is  added  to  the  stress  tensor  determined  from  the  strain  energy 
functional.   
If  we  wish  to  include  only  simple  rate  effects,  the  relaxation  function  is 
represented by six terms from the Prony series: 
𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚
𝑚=1
𝑒−𝛽𝑡,
(22.95.5)
given by,
LS-DYNA Theory Manual 
Material Models 
𝑔(𝑡) = ∑ 𝐺𝑖𝑒−𝛽𝑖𝑡
𝑖=1
.
(22.95.6)
This  model  is  effectively  a  Maxwell  fluid  which  consists  of  a  dampers  and  springs  in 
series.  We characterize this in the input by shear modulii, 𝐺𝑖, and decay constants, 𝛽𝑖.  
The viscoelastic behavior is optional and an arbitrary number of terms may be used.
Material Models 
LS-DYNA Theory Manual 
22.96  Material Model 128:  Heart Tissue 
This material model provides a tissue model described in the paper by Guccione, 
McCulloch, and Waldman [1991] 
The  tissue  model  is  described  in  terms  of  the  energy  functional  in  terms  of  the 
Green strain components, 𝐸𝑖𝑗, 
𝑊(𝐸, 𝐽) =
𝑄 = 𝑏1𝐸11
(𝑒𝑄 − 1) + 𝑊H(𝐽), 
2 + 𝐸33
2 + 𝑏2(𝐸22
2 + 𝐸23
2 + 𝐸32
2 ) + 𝑏3(𝐸12
2 + 𝐸21
2 + 𝐸13
2 + 𝐸31
2 ), 
(22.96.1)
where  the  hydrostatic  work  term  is  in  terms  of  the  bulk  modulus,  𝐾,  and  the  third 
invariant 𝐽, as: 
𝑊H(𝐽) =
(𝐽 − 1)2.
(22.96.2)
The  Green  components  are  modified  to  eliminate  any  effects  of  volumetric  work 
following the procedures of Ogden.
LS-DYNA Theory Manual 
Material Models 
22.97  Material Model 129:  Isotropic Lung Tissue 
This  material  model  provides  a  lung  tissue  model  described  in  the  paper  by 
Vawter [1980]. 
The material is described by a strain energy functional expressed in terms of the 
invariants of the Green Strain: 
𝑊(𝐼1, 𝐼2) =
𝐴2 =
2𝛥
(𝐼1 + 𝐼2) − 1,
𝑒(𝛼𝐼1
2+𝛽𝐼2) +
12𝐶1
𝛥(1 + 𝐶2)
[𝐴(1+𝐶2) − 1],
(22.97.1)
where  the  hydrostatic  work  term  is  in  terms  of  the  bulk  modulus,  𝐾,  and  the  third 
invariant 𝐽, as: 
𝑊H(𝐽) =
(𝐽 − 1)2,
(22.97.2)
Rate  effects  are  taken  into  account  through  linear  viscoelasticity  by  a  convolution 
integral of the form: 
𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙
(𝑡 − 𝜏)
𝜕𝜀𝑘𝑙
𝜕𝜏
𝑑𝜏,
(22.97.3)
or in terms of the second Piola-Kirchhoff stress, 𝑆𝑖𝑗, and Green's strain tensor, 𝐸𝑖𝑗, 
𝑆𝑖𝑗 = ∫ 𝐺𝑖𝑗𝑘𝑙
(𝑡 − 𝜏)
𝜕𝐸𝑘𝑙
𝜕𝜏
𝑑𝜏,
(22.97.4)
where  𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)  and  𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏)    are  the  relaxation  functions  for  the  different  stress 
measures.    This  stress  is  added  to  the  stress  tensor  determined  from  the  strain  energy 
functional.   
If  we  wish  to  include  only  simple  rate  effects,  the  relaxation  function  is 
represented by six terms from the Prony series: 
given by, 
𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚
𝑚=1
𝑒−𝛽𝑡,
𝑔(𝑡) = ∑ 𝐺𝑖𝑒−𝛽𝑖𝑡
𝑖=1
.
(22.97.5)
(22.97.6)
This  model  is  effectively  a  Maxwell  fluid  which  consists  of  a  dampers  and 
springs  in  series.    We  characterize  this  in  the  input  by  shear  moduli,  𝐺𝑖,  and  decay
Material Models 
LS-DYNA Theory Manual 
constants,  𝛽𝑖.    The  viscoelastic  behavior  is  optional  and  an  arbitrary  number  of  terms 
may be used.
LS-DYNA Theory Manual 
Material Models 
22.98  Material Model 130:  Special Orthotropic 
The in-plane elastic matrix for in-plane plane stress behavior is given by: 
𝐂in plane =
𝑄11p 𝑄12p
⎡
𝑄12p 𝑄22p
⎢
⎢
⎢
⎢
⎢
⎣
𝑄44p
𝑄55p
⎤
⎥
⎥
, 
⎥
⎥
⎥
𝑄66p⎦
where the terms 𝑄𝑖𝑗p are defined as: 
𝑄11p =
𝑄22p =   
𝑄12p =   
𝐸11p
1 − ν12pν21p
𝐸22p
1 − ν12pν21p
ν12pE11p
1 − ν12pν21p
,
, 
, 
𝑄44p = 𝐺12p, 
𝑄55p = 𝐺23p, 
Q66p = 𝐺31p.
The elastic matrix for bending behavior is given by: 
𝐂bending =
𝑄11b 𝑄12b
⎡
𝑄12b 𝑄22b
⎢
⎣
⎤
, 
⎥
𝑄44b⎦
(22.98.1)
(22.98.2)
(22.98.3)
where the terms 𝑄𝑖𝑗b are similarly defined.
Material Models 
LS-DYNA Theory Manual 
22.99  Material Model 131:  Isotropic Smeared Crack 
The  following  documentation  is  taken  nearly  verbatim  from  the  documentation 
of that by Lemmen and Meijer [2001]. 
Three methods are offered to model progressive failure.  The maximum principal 
stress  criterion  detects  failure  if  the  maximum  (most  tensile)  principal  stress  exceeds 
𝜎max.  Upon failure, the material can no longer carry stress. 
The second failure model is the smeared crack model with linear softening stress-
strain curve using equivalent uniaxial strains.  Failure is assumed to be perpendicular to 
the  principal  strain  directions.    A  rotational  crack  concept  is  employed  in  which  the 
crack directions are related to the current directions of principal strain.  Therefore crack 
directions may rotate in time.  Principal stresses are expressed as 
𝐸̅̅̅̅1
⎡
⎢⎢
⎣
𝐸̅̅̅̅1𝜀̃1
⎟⎟⎟⎞
𝐸̅̅̅̅2𝜀̃2
𝐸̅̅̅̅3𝜀̃3⎠
⎤
⎥⎥
𝐸̅̅̅̅3⎦
𝜎1
𝜎2
𝜎3⎠
𝜀̃1
𝜀̃2
𝜀̃3⎠
𝐸̅̅̅̅2
⎟⎟⎞ =
⎟⎞ =
⎜⎜⎜⎛
⎝
⎜⎜⎛
⎝
(22.99.1)
⎜⎛
⎝
, 
with 𝐸̅̅̅̅1, 𝐸̅̅̅̅2and 𝐸̅̅̅̅3 being secant stiffness in the terms that depend on internal variables. 
In  the  model  developed  for  DYCOSS  it  has  been  assumed  that  there  is  no 
interaction between the three directions in which case stresses simply follow  
𝜎𝑗(𝜀̃𝑗) =
⎧
{
{
{
{
{
⎨
{
{
{
{
{
⎩
𝐸𝜀̃𝑗
if
0 ≤ 𝜀̃𝑗 ≤ 𝜀̃𝑗,ini
(1 −
𝜀̃𝑗 − 𝜀̃𝑗,ini
𝜀̃𝑗,ult − 𝜀̃𝑗,ini
) 𝜎̅̅̅̅̅
if
𝜀̃𝑗,ini < 𝜀̃𝑗 ≤ 𝜀̃𝑗,ult
, 
(22.99.2)
if
𝜀̃𝑗 > 𝜀̃𝑗,ult
with 𝜎̅̅̅̅̅ the ultimate stress, 𝜀̃𝑗,ini the damage threshold, and 𝜀̃𝑗,ultthe ultimate strain in 𝑗-
direction.  The damage threshold is defined as 
𝜀̃𝑗,ini =
𝜎̅̅̅̅̅
.
(22.99.3)
The  ultimate  strain  is  obtained  by  relating  the  crack  growth  energy  and  the 
dissipated energy 
∫ ∫ 𝜎̅̅̅̅̅ 𝑑𝜀̃𝑗,ult 𝑑𝑉 = 𝐺𝐴,
(22.99.4)
with 𝐺 the energy release rate, 𝑉 the element volume and 𝐴 the area perpendicular to 
the  principal  strain  direction.    The  one-point  elements  in  LS-DYNA  have  a  single
LS-DYNA Theory Manual 
Material Models 
integration point and the integral over the volume may be replaced by the volume.  For 
linear softening it follows 
𝜀̃𝑗,ult =
2𝐺𝐴
,
𝑉𝜎̅̅̅̅̅
(22.99.5)
The  above  formulation  may  be  regarded  as  a  damage  equivalent  to  the 
maximum principle stress criterion. 
The third model is a damage model presented by Brekelmans et.  al. [1991].  Here 
the Cauchy stress tensor 𝜎 is expressed as 
𝜎 = (1 − 𝐷)𝐸𝜀,
(22.99.6)
where  𝐷  represents  the  current  damage  and  the  factor  (1 − 𝐷)  is  the  reduction  factor 
caused by damage.  The scalar damage variable is expressed as a function of a so-called 
damage equivalent strain 𝜀d 
𝐷 = 𝐷(𝜀d) = 1 −
𝜀ini(𝜀ult − 𝜀d)
𝜀d(𝜀ult − 𝜀ini)
,
with ultimate and initial strains as defined by 
𝜀d =
𝑘 − 1
2𝑘(1 − 2𝑣)
𝐽1 +
2𝑘
√(
𝑘 − 1
1 − 2𝑣
𝐽1)
+
6𝑘
(1 + 𝑣)2 𝐽2,
(22.99.7)
(22.99.8)
where the constant 𝑘 represents the ratio of the strength in tension over the strength in 
compression 
𝑘 =
𝜎ult,tension
𝜎ult,compression
,
(22.99.9)
𝐽1  and  𝐽2  are  the  first  and  the  second  invariants  of  the  strain  tensor  representing  the 
volumetric and the deviatoric straining, respectively 
𝐽1 = 𝜀𝑖𝑗,
′ 𝜀𝑖𝑗
′ ,
𝐽2 = 𝜀𝑖𝑗
(22.99.10)
where 𝜀𝑖𝑗
′  denotes the deviatoric part of the strain tensor. 
If  the  compression  and  tension  strength  are  equal  the  dependency  on  the 
volumetric strain vanishes in Equation (22.99.8) and failure is shear dominated.  If the 
compressive strength is much larger than the strength in tension, 𝑘 becomes large and 
the 𝐽1 terms in Equation (22.99.8) dominate the behavior.
Material Models 
LS-DYNA Theory Manual 
22.100  Material Model 133:  Barlat_YLD2000 
The yield condition for this material can be written 
𝑓 (𝜎, 𝛼, 𝜀p) = 𝜎eff(𝜎𝑥𝑥 − 2𝛼𝑥𝑥 − 𝛼𝑦𝑦, 𝜎𝑦𝑦 − 2𝛼𝑦𝑦 − 𝛼𝑥𝑥, 𝜎𝑥𝑦 − 𝛼𝑥𝑦) −
                        𝜎Y
t (𝜀p, 𝜀̇p, 𝛽) ≤ 0,
(22.100.1)
where 
(𝜑′ + 𝜑′′)
𝜎eff(𝑠𝑥𝑥, 𝑠𝑦𝑦, 𝑠𝑥𝑦) =
𝜑′ = ∣𝑋′1 − 𝑋′2∣𝑎, 
𝜑′′ = ∣2𝑋′′1 + 𝑋′′2∣𝑎 + ∣𝑋′′1 + 2𝑋′′2∣𝑎.
, 
⎟⎞
⎠
⎜⎛1
⎝
The 𝑋′𝑖 and 𝑋′′𝑖 are the eigenvalues of 𝑋′𝑖𝑗 and 𝑋′′𝑖𝑗 and are given by  
𝑋′1 =
𝑋′2 =
(𝑋′11 + 𝑋′22 + √(𝑋′11 − 𝑋′22)2 + 4𝑋′12
2 ) ,
(𝑋′11 + 𝑋′22 − √(𝑋′11 − 𝑋′22)2 + 4𝑋′12
2 ),
and  
𝑋′′1 =
𝑋′′2 =
(𝑋′′11 + 𝑋′′22 + √(𝑋′′11 − 𝑋′′22)2 + 4𝑋′′12
2 ) , 
(𝑋′′11 + 𝑋′′22 − √(𝑋′′11 − 𝑋′′22)2 + 4𝑋′′12
2 ),
respectively.  The 𝑋′𝑖𝑗 and 𝑋′′𝑖𝑗 are given by4 
𝑋′11
⎟⎟⎟⎞
⎜⎜⎜⎛
𝑋′22
𝑋′12⎠
⎝
𝑋′′11
𝑋′′22
𝑋′′12⎠
⎜⎛
⎝
=
⎜⎜⎜⎛
⎝
𝐿′11 𝐿′12
𝐿′21 𝐿′22
𝐿′′11 𝐿′′12
𝐿′′21 𝐿′′22
⎜⎛
⎝
⎟⎞ =
⎟⎟⎟⎞
𝐿′33⎠
⎟⎞
𝐿′′33⎠
⎜⎛
⎝
𝑠𝑥𝑥
⎟⎞ , 
𝑠𝑦𝑦
𝑠𝑥𝑦⎠
𝑠𝑥𝑥
𝑠𝑦𝑦
𝑠𝑥𝑦⎠
⎜⎛
⎝
⎟⎞, 
where 
⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞
𝐿′11
𝐿′12
𝐿′21
𝐿′22
𝐿′33⎠
⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛
⎝
=
−1
0 −1
⎜⎜⎜⎜⎜⎜⎜⎛
⎝
⎟⎟⎟⎟⎟⎟⎟⎞
3⎠
𝛼1
𝛼2
𝛼7⎠
⎟⎞ , 
⎜⎛
⎝
(22.100.2)
(22.100.3)
(22.100.4)
(22.100.5)
(22.100.6)
LS-DYNA Theory Manual 
Material Models 
𝐿′′11
𝐿′′12
𝐿′′21
𝐿′′22
𝐿′′33⎠
⎟⎟⎟⎟⎟⎟⎟⎞
⎜⎜⎜⎜⎜⎜⎜⎛
⎝
=
−2
1 −4 −4
4 −4 −4
−2
8 −2
2 −2
⎜⎜⎜⎜⎜⎜⎜⎛
⎝
⎟⎟⎟⎟⎟⎟⎟⎞
9⎠
⎟⎟⎟⎟⎟⎟⎟⎞
𝛼3
𝛼4
𝛼5
𝛼6
𝛼8⎠
⎜⎜⎜⎜⎜⎜⎜⎛
⎝
. 
where 𝛼1 to 𝛼8 are the parameters that determine the shape of the yield surface.  
The yield stress is expressed as 
t (𝜀p, 𝜀̇p, 𝛽) = 𝜎Y
𝜎Y
v(𝜀p, 𝜀̇p) + 𝛽(𝜎0 − 𝜎Y
v(𝜀p, 𝜀̇p)),
(22.100.7)
where  𝛽  determines  the  fraction  kinematic  hardening  and 𝜎0  is  the  initial  yield  stress.  
The yield stress for purely isotropic hardening is given by 
v(𝜀p, 𝜀̇p) = 𝜎Y(𝜀p)
𝜎Y
1 + {
⎜⎜⎜⎛
⎝
𝜀̇p
}
, 
⎟⎟⎟⎞
⎠
(22.100.8)
where 𝐶 and 𝑝 are the Cowper-Symonds material parameters for strain rate effects.  
The evolution of back stress is given by 
⎜⎛∂𝜎Y
∂𝜀p ⎝
⎜⎛1 + {
𝛼̇ = 𝜆̇𝛽 ⎝
𝜀̇p
}
1/𝑝−1
𝑝𝐶Δ𝑡
𝜀̇p
{
}
1/p
⎟⎞ + 𝜎Y
⎠
∂𝜎eff
∂𝑠
∂𝜎eff
∂𝑠
⋅
⎟⎞
⎠
∂𝜎eff
∂𝑠
, 
(22.100.9)
where Δ𝑡 is the current time step size and 𝜆̇ is the rate of plastic strain multiplier. 
For the plastic return algorithms, the gradient of effective stress is computed as 
∂𝜎eff
∂𝑠xx
∂𝜎eff
∂𝑠yy
∂𝜎eff
∂𝑠xy ⎠
⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞
⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛
⎝
=
𝑎−1
𝑎𝜎eff
L′11 L′21
L′12 L′22
⎜⎜⎜⎛
⎝
⎟⎟⎟⎞
L′33⎠
⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛
⎝
𝜕𝜙′
𝜕𝑋′11
𝜕𝜙′
𝜕𝑋′22
𝜕𝜙′
𝜕𝑋′12⎠
+
𝑎−1
𝑎𝜎eff
L′′11 L′′21
L′′12 L′′22
⎜⎜⎜⎛
⎝
⎟⎟⎟⎞
L′′33⎠
⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞
⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛
∂𝜙′′
∂X′′11
∂𝜙′′
∂X′′22
∂𝜙′′
∂X′′12⎠
⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞
with the aid of 
⎝
(22.100.10)
,
Material Models 
LS-DYNA Theory Manual 
𝜕𝜑′
𝜕𝑋′𝑖𝑗
= 𝑎(𝑋′1 − 𝑋′2)𝑎−1 𝜕(𝑋′1 − 𝑋′2)
𝜕𝑋′𝑖𝑗
, 
𝜕𝜑′′
𝜕𝑋′′𝑖𝑗
= 𝑎∣2𝑋′′1 + 𝑋′′2∣𝑎−1sgn(2𝑋′′1 + 𝑋′′2)
                𝑎∣2𝑋′′2 + 𝑋′′1∣𝑎−1sgn(2𝑋′′2 + 𝑋′′1)
𝜕(2𝑋′′1 + 𝑋′′2)
𝜕𝑋′′𝑖𝑗
𝜕(2𝑋′′2 + 𝑋′′1)
𝜕𝑋′′𝑖𝑗
+
,
and 
𝜕(𝑋′1 − 𝑋′2)
𝜕𝑋′11
=
𝑋′11 − 𝑋′22
√(𝑋′11 − 𝑋′22)2 + 4𝑋′12
,
𝜕(𝑋′1 − 𝑋′2)
𝜕𝑋′22
=
𝑋′22 − 𝑋′11
√(𝑋′11 − 𝑋′22)2 + 4𝑋′12
,
𝜕(𝑋′1 − 𝑋′2)
𝜕𝑋′12
=
4𝑋′12
√(𝑋′11 − 𝑋′22)2 + 4𝑋′12
,
𝜕(2𝑋′′1 + 𝑋′′2)
𝜕𝑋′′11
=
𝜕(2𝑋′′1 + 𝑋′′2)
𝜕𝑋′′22
=
+
𝑋′′11 − 𝑋′′22
√(𝑋′′11 − 𝑋′′22)2 + 4𝑋′′12
,
+
𝑋′′22 − 𝑋′′11
√(𝑋′′11 − 𝑋′′22)2 + 4𝑋′′12
,
𝜕(2𝑋′′1 + 𝑋′′2)
𝜕𝑋′′12
=
2𝑋′′12
√(𝑋′′11 − 𝑋′′22)2 + 4𝑋′′12
,
(22.100.11)
(22.100.12)
(22.100.13) 
(22.100.14) 
(22.100.15) 
(22.100.16) 
(22.100.17) 
(22.100.18) 
𝜕(2𝑋′′2 + 𝑋′′1)
𝜕𝑋′′11
=
−
𝑋′′11 − 𝑋′′22
√(𝑋′′11 − 𝑋′′22)2 + 4𝑋′′12
,
(22.100.19) 
𝜕(2𝑋′′2 + 𝑋′′1)
𝜕𝑋′′22
=
−
𝑋′′22 − 𝑋′′11
√(𝑋′′11 − 𝑋′′22)2 + 4𝑋′′12
,
(22.100.20)
𝜕(2𝑋′′2 + 𝑋′′1)
𝜕𝑋′′12
= −
2𝑋′′12
√(𝑋′′11 − 𝑋′′22)2 + 4𝑋′′12
.
(22.100.21)
The algorithm for the plane stress update as well as the formula for the tangent 
modulus is given in detail in Section 19.36.1 and is not repeated here.
LS-DYNA Theory Manual 
Material Models 
22.100.1  Closest point projection algorithm 
This  section  describes  shortly  the  closest  point  projection  algorithm  that  was 
implemented to improve accuracy, hence the implicit performance, of the model.  The 
closest point projection comes down to solving the following system of equations 
𝑓1 = 𝑡 + 𝐀𝛼 + (𝛔Y
t (Δ𝜆) − 𝛔Y
t (0))ℎ − 𝛔trial(Δ𝜀33) + 2𝐺Δ𝜆D∇𝜎eff(t) = 0, 
𝑓2 = −𝛔eff(t) + 𝛔Y
t (Δ𝜆) = 0,
𝑓3 = 𝜎33
trial(Δ𝜀33) + 2𝐺Δ𝜆(∇𝜎eff
1 (t) + ∇𝜎eff
2 (t)) = 0,
where 
ℎ =
∇𝜎eff(𝑡)T𝐁∇𝜎eff(𝑡)
𝐁∇𝜎eff(𝑡),
(22.100.22)
(22.100.23)
(22.100.24)
(22.100.25)
in  terms  of  the  unknown  variables  𝐭  (stress),  Δε33  (thickness  strain  increment)  and  Δ𝜆 
(plastic strain increment).  In the above 
𝐃 =
⎡
⎢
⎣
⎤ ,    𝐀 =
⎥
0.5⎦
⎡
⎢
⎣
⎤ ,    𝐁 =
⎥
1 ⎦
⎡
⎢
⎣
⎤ ,    𝐻 =
⎥
0.5⎦
∂σY
∂εp
. 
(22.100.26)
This  system  of  equations  is  solved  using  a  Newton  method  with  an  additional 
line search for robustness.  Using the notation 
𝐟 =
𝑓1
⎤
𝑓2
⎥
𝑓3⎦
⎡
⎢
⎣
,    𝐱 =
⎤, 
⎡
Δ𝜆
⎥
⎢
Δ𝜀33⎦
⎣
a Newton step is completed as 
𝑥+ = 𝑥− − 𝑠 (
∂𝑓
∂𝑥
−1
)
(22.100.27)
(22.100.28)
for  a  step  size 𝑠 ≤ 1  chosen  such  that  the  norm  of  the  objective  function  is  decreasing.  
The gradient of the objective function is given by 
∇𝑓 = ∇𝑓1−β + ∇𝑓β
(22.100.29)
where 
∇f1−β =
I + 2𝐺Δ𝜆𝐷∇2𝜎eff
⎡
−(∇𝜎eff)T
⎢⎢
2𝐺Δ𝜆𝐞T∇2𝛔eff
⎣
2𝐺𝐷∇𝜎eff −𝐶3
⎤
⎥⎥
2GeT∇σeff C33 ⎦
(22.100.30)
Material Models 
LS-DYNA Theory Manual 
∇fβ =
∂h
∂𝑡
⎡Δ𝜆𝐻
⎢⎢⎢
0T
⎣
𝐻ℎ
⎤
⎥⎥⎥
0⎦
and 
𝐞 =
⎥⎤,    C3 = (K −
⎢⎡
0⎦
⎣
2G
) e, C33 = (K +
4G
),
(22.100.31)
(22.100.32)
𝐺 and 𝐾 stands for the shear and bulk modulus, respectively.  This algorithm requires 
computation  of  the  effective  stress  hessian.    The  derivation  of  this  is  quite  straightfor-
ward but the expression for it is rather long and is hence omitted in this report.
LS-DYNA Theory Manual 
Material Models 
22.101  Material Model 134:  Viscoelastic Fabric 
The  viscoelastic  fabric  model  is  a  variation  on  the  general  viscoelastic  Material 
Model  76.    This  model  is  valid  for  3  and  4  node  membrane  elements  only  and  is 
strongly recommended for modeling isotropic viscoelastic fabrics where wrinkling may 
be  a  problem.    For  thin  fabrics,  buckling  can  result  in  an  inability  to  support 
compressive  stresses;  thus,  a  flag  is  included  for  this  option.    If  bending  stresses  are 
important, use a shell formulation with Model 76. 
Rate effects are taken into account through linear viscoelasticity by a convolution 
integral of the form: 
𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙
(𝑡 − 𝜏)
𝜕𝜀𝑘𝑙
𝜕𝜏
𝑑𝜏,
(22.101.1)
where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)  is the relaxation function. 
If  we  wish  to  include  only  simple  rate  effects  for  the  deviatoric  stresses,  the 
relaxation function is represented by six terms from the Prony series: 
𝑔(𝑡) = ∑ 𝐺𝑚
𝑚=1
𝑒−𝛽𝑚𝑡.
(22.101.2)
We  characterize  this  in  the  input  by  shear  modulii,  𝐺𝑖,  and  decay  constants,  𝛽𝑖.    An 
arbitrary number of terms, up to 6, may be used when applying the viscoelastic model.  
For  volumetric  relaxation,  the  relaxation  function  is  also  represented  by  the 
Prony series in terms of bulk modulii: 
𝑘(𝑡) = ∑ 𝐾𝑚
𝑚=1
𝑒−𝛽𝑘𝑚𝑡.
(22.101.3)
Material Models 
LS-DYNA Theory Manual 
22.102  Material Model 139:  Modified Force Limited 
This material model is available for the Belytschko resultant beam element only.  
Plastic  hinges  form  at  the  ends  of  the  beam  when  the  moment  reaches  the  plastic 
moment.  The plastic moment versus rotation relationship is specified by the user in the 
form of a load curve and scale factor.  The points of the load curve are (plastic rotation 
in radians, plastic moment).  Both quantities should be positive for all points, with the 
first  point  being  (zero,  initial  plastic  moment).    Within  this  constraint  any  form  of 
characteristic  may  be  used,  including  flat  or  falling  curves.    Different  load  curves  and 
scale factors may be specified at each node and about each of the local s and t axes. 
Axial collapse occurs when the compressive axial load reaches the collapse load.  
Collapse  load  versus  collapse  deflection  is  specified  in  the  form  of  a  load  curve.    The 
points  of  the  load  curve  are  either  (true  strain,  collapse  force)  or  (change  in  length, 
collapse force).  Both quantities should be entered as positive for all points, and will be 
interpreted as compressive.  The first point should be (zero, initial collapse load). 
The collapse load may vary with end moment as well as with deflections.  In this 
case  several  load-deflection  curves  are  defined,  each  corresponding  to  a  different  end 
moment.    Each  load  curve  should  have  the  same  number  of  points  and  the  same 
deflection values.  The end moment is defined as the average of the absolute moments 
at each end of the beam and is always positive. 
Stiffness-proportional damping may be added using the damping factor 𝜆.  This 
is defined as follows: 
𝜆 =
2 ∗ 𝜉
,
(22.102.1)
where 𝜉  is the damping factor at the reference frequency 𝜔 (in radians per second).  For 
example if 1% damping at 2Hz is required 
𝜆 =
2 ∗ 0.01
2π ∗ 2
= 0.001592.
(22.102.2)
If damping is used, a small time step may be required.  LS-DYNA does not check this so 
to  avoid  instability  it may  be  necessary  to  control  the  timestep via  a  load  curve.   As a 
guide,  the  timestep  required  for  any  given  element  is  multiplied  by  0.3𝐿/𝑐𝜆  when 
damping is present (𝐿 = element length, 𝑐 = sound speed). 
Moment Interaction 
Plastic hinges can form due to the combined action of moments about the three 
axes.    This  facility  is  activated  only  when  yield  moments  are  defined  in  the  material 
input.  A hinge forms when the following condition is first satisfied.
LS-DYNA Theory Manual 
Material Models 
(
𝑀r
𝑀ryield
)
+ (
𝑀s
𝑀syield
)
+ (
𝑀t
𝑀tyield
)
≥ 1,
(22.102.3)
where, 
𝑀r, 𝑀s, 𝑀t= current moments 
𝑀ryield, 𝑀syield, 𝑀tyield= yield moments 
Note that scale factors for hinge behavior defined in the input will also be applied to the 
yield  moments:    for  example,  𝑀syield  in  the  above formula  is  given  by  the  input  yield 
moment about the local axis times the input scale factor for the local s-axis.  For strain-
softening  characteristics,  the  yield  moment  should  generally  be  set  equal  to  the  initial 
peak of the moment-rotation load curve. 
On forming a hinge, upper limit moments are set.  These are given by  
𝑀rupper = MAX
⎜⎛𝑀r,
⎝
𝑀ryield
⎟⎞,
2 ⎠
(22.102.4)
and similarly for 𝑀s and 𝑀t.  Thereafter the plastic moments will be given by: 
𝑀rp = min (𝑀rcurve, 𝑀rcurve)  
and similarly for 𝑠 and 𝑡, where 
𝑀rp = current plastic moment 
𝑀rcurve = moment taken from load curve at the current rotation scaled according 
to the scale factor. 
The  effect  of  this  is  to  provide  an  upper  limit  to  the  moment  that  can  be 
generated;  it represents  the  softening  effect  of  local  buckling  at  a  hinge  site.   Thus  if  a 
member is bent about its local s-axis it will then be weaker in torsion and about its local 
𝑡-axis.  For moment-softening curves, the effect is to trim off the initial peak (although if 
the curves subsequently harden, the final hardening will also be trimmed off). 
It is not possible to make the plastic moment vary with the current axial load, but 
it  is  possible  to  make  hinge  formation  a  function  of  axial  load  and  subsequent  plastic 
moment a function of the moment at the time the hinge formed.  This is discussed in the 
next section. 
Independent plastic hinge formation 
In addition to the moment interaction equation, Cards 7 through 18 allow plastic 
hinges to form independently for the s-axis and t-axis at each end of the beam and also 
for  the  torsional  axis.    A  plastic  hinge  is  assumed  to  form  if  any  component  of  the 
current  moment  exceeds  the  yield  moment  as  defined  by  the  yield  moment  vs.    axial 
force curves input on cards 7 and 8.  If any of the 5 curves is omitted, a hinge will not 
form for that component.  The curves can be defined for both compressive and tensile 
axial forces.  If the axial force falls outside the range of the curve, the first or last point in 
the curve will be used.  A hinge forming for one component of moment does not affect 
the other components.
Material Models 
LS-DYNA Theory Manual 
Upon forming a hinge, the magnitude of that component of moment will not be 
permitted  to  exceed  the  current  plastic  moment.    The  current  plastic  moment  is 
obtained by interpolating between the plastic moment vs.  plastic rotation curves input 
on cards 10, 12, 14, 16, or 18.  Curves may be input for up to 8 hinge moments, where 
the  hinge  moment  is  defined  as  the  yield  moment  at  the  time  that  the  hinge  formed.  
Curves must be input in order of increasing hinge moment and each curve should have 
the same plastic rotation values.  The first or last curve will be used if the hinge moment 
falls  outside  the  range  of  the  curves.    If  no  curves  are  defined,  the  plastic  moment  is 
obtained  from  the  curves  on  cards  4  through  6.    The  plastic  moment  is  scaled  by  the 
scale factors on lines 4 to 6. 
A  hinge  will  form  if  either  the  independent  yield  moment  is  exceeded  or  if  the 
moment interaction equation is satisfied.  If both are true, the plastic moment will be set 
to the minimum of the interpolated value and 𝑀rp.
M8
M7
M6
M5
M4
M3
M2
M1
Strain (or change in length, see AOPT)
Figure 22.102.1.  The force magnitude is limited by the applied end moment.
For an intermediate value of the end moment LS-DYNA interpolates between 
the curves to determine the allowable force value.
LS-DYNA Theory Manual 
Material Models 
22.103  Material Model 141:  Rate Sensitive Polymer  
𝜀𝑖𝑗 = 𝐷oexp [−
(
𝑍o
3𝐾2
)]
𝑆𝑖𝑗 − 𝛺𝑖𝑗
⎟⎞,
√𝐾2 ⎠
⎜⎛
⎝
(22.103.1)
where  𝐷o  is  the  maximum  inelastic  strain  rate,  𝑍o  is  the  isotropic  initial  hardness  of 
material,  𝛺𝑖𝑗  is  the  internal  stress,  𝑆𝑖𝑗  is  the  deviatoric  stress  component,  and  𝐾2  is 
defined as follows: 
𝐾2 =
(𝑆𝑖𝑗 − 𝛺𝑖𝑗)(𝑆𝑖𝑗 − 𝛺𝑖𝑗),
(22.103.2)
and represent the second invariant of the overstress tensor.  The elastic components of 
the  strain  are  added  to  the  inelastic  strain  to  obtain  the  total  strain.    The  following 
relationship defines the internal stress variable rate: 
𝛺𝑖𝑗 =
𝑞𝛺m𝜀̇𝑖𝑗
I ,
I − 𝑞𝛺𝑖𝑗𝜀̇e
(22.103.3)
where 𝑞 is a material constant, 𝛺m is a material constant that represents the maximum 
value of the internal stress, and 𝜀̇e
I  is the effective inelastic strain.
Material Models 
LS-DYNA Theory Manual 
22.104  Material Model 142: Transversely Anisotropic 
Crushable Foam 
A  new  material  model  for  low  density,  transversely  isotropic  crushable  foams, 
has been developed at DaimlerChrysler by Hirth, Du Bois, and Weimar.  Hirth, Du Bois, 
and  Weimar  determined  that  material  model  26,  MAT_HONEYCOMB,  which  is 
commonly used to model foams, can systematically over estimate the stress when it is 
loaded  off-axis.    Their  new  material  model  overcomes  this  problem  without  requiring 
any additional input.  Their new model can possibly replace the MAT_HONEYCOMB 
material, which is currently used in the frontal offset and side impact barriers. 
Many  polymers  used  for  energy  absorption  are  low  density,  crushable  foams 
with  no  noticeable  Poisson  effect.    Frequently  manufactured  by  extrusion,  they  are 
transversely  isotropic.    This  class  of  material  is  used  to  enhance  automotive  safety  in 
low velocity (bumper impact) and medium velocity (interior head impact) applications.  
These materials require a transversely isotropic, elastoplastic material with a flow rule 
allowing for large permanent volumetric deformations.   
The  MAT_HONEYCOMB  model  uses  a  local  coordinate  system  defined  by  the 
user.  One of the axes of the local system coincides  with the extrusion direction of the 
honeycomb  in  the  undeformed  configuration.    As  an  element  deforms,  its  local 
coordinate  system  rotates  with  its  mean  rigid  body  motion.    Each  of  the  six  stress 
components is treated independently, and each has its own law relating its flow stress 
to its plastic strain. 
The  effect  of  off-axis  loading  on  the  MAT_HONEYCOMB  model  can  be 
estimated  by  restricting  our  considerations  to  plane  strain  in  two  dimensions.    Our 
discussion is restricted to the response of the foam before it becomes fully compacted.  
After  compaction,  its  response  is  modeled  with  conventional  𝐽2  plasticity.    The  model 
reduces to  
y (𝜀V),
y (𝜀V), 
y (𝜀V),
where 𝜀V is the volumetric strain.  For a fixed value of volumetric strain, the individual 
stress components respond in an elastic-perfectly plastic manner, i.e., the foam doesn’t 
have any strain hardening.  
|σ11| ≤ 𝜎11
|𝜎22| ≤ 𝜎22
|𝜎12| ≤ 𝜎12
(22.104.1)
In two dimensions, the stress tensor transforms according to 
[𝜎] = [𝑅(𝜃)]T[𝜎𝜃][𝑅(𝜃)],
(22.104.2)
LS-DYNA Theory Manual 
Material Models 
[𝑅(𝜃)] = [
cos(𝜃) − sin(𝜃)
cos(𝜃)
sin(𝜃)
],
where  𝜃  is  the  angle  of  the  local  coordinate  system  relative  to  the  global  system.    For 
uniaxial loading along the global 1-axis, the stress will be (accounting for the sign of the 
volume strain), 
𝜎11 = {[cos(𝜃)]2𝜎11
y + [sin(𝜃)]2𝜎22
y + 2 ⋅ sin(𝜃)cos(𝜃)𝜎12
y }sgn(𝜀V)}, 
(22.104.3)
assuming the strain is large enough to cause yielding in both directions. 
y  
y   and  𝜎22
If  the  shear  strength  is  neglected,  𝜎11  will  vary  smoothly  between  𝜎11
and  never  exceed  the maximum  of  the  two  yield  stresses.    This  behavior  is  intuitively 
what  we  would  like  to  see.    However,  if  the  value  of  shear  yield  stress  isn’t  zero,  𝜎11 
y  are equal (a nominally 
y . To illustrate, if 𝜎11
will be greater than either 𝜎11
isotropic response) the magnitude of the stress is 
y  and 𝜎22
y  or 𝜎22
|𝜎11| = 𝜎11
y ,
y + 2 ⋅ sin(𝜃)cos(𝜃)𝜎12
and achieves a maximum value at 45 degrees of  
y .
y + 𝜎12
|𝜎11| = 𝜎11
(22.104.4)
(22.104.5)
For cases where there is anisotropy, the maximum occurs at a different angle and 
will  have  a  different magnitude,  but  it  will  exceed  the  maximum  uniaxial  yield  stress.  
In fact, a simple calculation using Mohr’s circle shows that the maximum value will be 
y =
𝜎max
(𝜎11
y + 𝜎22
y ) +
√(𝜎11
y )
y − 𝜎22
y ,
+ 4𝜎12
(22.104.6)
To  correct  for  the  systematic  overestimation  of  the  off-axis  strength  by  MAT_ 
HONEYCOMB,  MAT_TRANSVERSELY_ISOTROPIC_CRUSHABLE_FOAM  has  been 
implemented in LS-DYNA.  It uses a single yield surface, calculated dynamically from 
the six yield stresses specified by the user.  The yield surface hardens and softens as a 
function  of  the  volumetric  strain  through  the  yield  stress  functions.    While  the  cost  of 
the model is higher than for MAT_HONEYCOMB, its superior response off-axis makes 
it  the  model  of  choice  for  critical  applications  involving  many  types  of  low-density 
foams.
Material Models 
LS-DYNA Theory Manual 
22.105  Material Model 143:  Wood Model 
The  wood  model  is  a  transversely  isotropic  material  and  is  available  for  solid 
elements.    The  development of  this  model  was  done  by  Murray  [2002],  who  provided 
the documentation that follows, under a contract from the FHWA.   
The general constitutive relation for an orthotropic material, written in terms of 
the principal material directions [Bodig & Jayne, 1993] is: 
𝜎1
⎤
⎡
𝜎2
⎥
⎢
𝜎3
⎥
⎢
⎥
⎢
𝜎4
⎥
⎢
⎥
⎢
𝜎5
𝜎6⎦
⎣
  =
𝐶11 𝐶12 𝐶13
⎡
𝐶21 𝐶22 𝐶23
⎢
⎢
𝐶31 𝐶32 𝐶33
⎢
⎢
⎢
⎢
⎣
2𝐶44
2𝐶55
⎤
⎥
⎥
⎥
⎥
⎥
⎥
2𝐶66⎦
=
𝜀1
⎤
⎡
𝜀2
⎥
⎢
𝜀3
⎥
⎢
⎥
⎢
𝜀4
⎥
⎢
⎥
⎢
𝜀5
𝜀6⎦
⎣
. 
(22.105.1)
The subscripts 1, 2, and 3 refer to the longitudinal, tangential, and radial, stresses and 
strains  (1 = 11,2 = 22,3 = 33,1 = 11,2 = 22,3 = 33),  respectively. 
  The 
subscripts 4, 5, and 6 are in a shorthand notation that refers to the shearing stresses and 
strains  4 = 12,5 =  13,6 = 23,4 = 12,5 = 13,6 = 23).  As  an  alternative 
notation for wood, it is common to substitute L (longitudinal) for 1, T (tangential) for 2, 
and  R  (radial)  for  3.  The  components  of  the  constitutive  matrix,  𝐶𝑖𝑗,  are  listed  here  in 
terms of the nine independent elastic constants of an orthotropic material:  
C11 =  
C22 =
C33 =
C12 =
C13 =
,
, 
E11(1  −   ν23ν32)
E22(1  −   ν31ν13)
E33(1  −   ν12ν21)
, 
(ν21   +   ν31ν23)E11
(ν31   +   ν21ν32)E11
(ν32   +   ν12ν31)E22
C23 =
C44 = G12, 
C55 = G13, 
C66 = G23, 
, 
, 
, 
(22.105.2)
Δ = 1 − ν12ν21 − ν23ν32 − ν31ν13 − 2ν21ν32ν13.
The  following  identity,  relating  the  dependent  (minor  Poisson’s  ratios  ν21,  ν31, 
and  ν32) and independent elastic constants, is obtained from symmetry considerations 
of the constitutive matrix:
LS-DYNA Theory Manual 
Material Models 
𝜈𝑖𝑗
𝐸𝑖
=
𝜈𝑗𝑖
𝐸𝑗
for
𝑖, 𝑗 = 1, 2, 3.
(22.105.3)
One common assumption is that wood materials are transversely isotropic.  This 
means that the properties in the tangential and radial directions are modeled the same, 
i.e. 𝐸22 =   𝐸33, 𝐺12 = 𝐺13, and 12 = 13.  This reduces the number of independent elastic 
constants  to  five,  𝐸11, 𝐸22,12, 𝐺12,  and  𝐺23.    Further,  Poisson's  ratio  in  the  isotropic 
plane, 23,  is  not  an  independent  quantity.    It  is  calculated  from  the  isotropic  relation: 
= (𝐸 − 2𝐺)/2𝐺 where E = 𝐸22 =   𝐸33 and 𝐺 = 𝐺23. Transverse isotropy is a reasonable 
assumption because the difference between the tangential and radial properties of wood 
(particularly  Southern  yellow  pine  and  Douglas  fir)  is  small  in  comparison  with  the 
difference between the tangential and longitudinal properties.  
The  yield  surfaces  parallel  and  perpendicular  to  the  grain  are  formulated  from 
six  ultimate  strength  measurements  obtained  from  uniaxial  and  pure-shear  tests  on 
wood specimens:  
XT 
XC 
YT 
YC 
S|| 
S⊥ 
Tensile strength parallel to the grain 
Compressive strength parallel to the grain 
Tensile strength perpendicular to the grain 
Compressive strength perpendicular to the grain 
Shear strength parallel to the grain 
Shear strength perpendicular to the grain 
Here  𝑋  and  𝑌  are  the  strengths  parallel  and  perpendicular  to  the  grain, 
respectively,  and  S  are  the  shear  strengths.    The  formulation  is  based  on  the  work  of 
Hashin [1980]. 
For  the  parallel  modes,  the  yield  criterion  is  composed  of  two  terms  involving 
two  of  the  five  stress  invariants  of  a  transversely  isotropic  material.    These  invariants 
2   This criterion predicts that the normal and shear stresses 
are 𝐼1 = 𝜎11 and 𝐼4 = 𝜎12
are mutually weakening, i.e. the presence of shear stress reduces the strength below that 
measured in uniaxial stress tests.  Yielding occurs when 𝑓||   ≥  0, where:  
2 + 𝜎13
𝑓|| =
𝜎11
𝑋2 +
(𝜎12
2 )
2 + 𝜎13
𝑆||
− 1
𝑋 = {
𝑋𝑡
𝑋𝑐
for 
for
𝜎11 > 0
𝜎11 < 0
. 
(22.105.4)
For the  perpendicular modes,  the  yield  criterion  is  also  composed  of  two  terms 
involving  two  of  the  five  stress  invariants  of  a  transversely  isotropic  material.    These 
2 − 𝜎22𝜎33.  Yielding occurs when 𝑓  0, where: 
invariants are 𝐼2 =  22 + 33 and 𝐼3 = 𝜎23
𝑓⊥ =
(𝜎22 + 𝜎33)2
𝑌2
+
(𝜎23
2 − 𝜎22𝜎33)
𝑆⊥
− 1
𝑌 = {
𝑌t
𝑌c
for
for
𝜎22 + 𝜎33 > 0
𝜎22 + 𝜎33 < 0
(22.105.5)
Material Models 
LS-DYNA Theory Manual 
Figure  22.105.1.    The  yield  criteria  for  wood  produces  smooth  surfaces  in 
stress space. 
Each  yield  criterion  is  plotted  in  3D  in  Figure  22.105.1  in  terms  of  the  parallel  and 
perpendicular stresses.  Each criterion is a smooth surface (no corners). 
The  plasticity  algorithms  limit  the  stress  components  once  the  yield  criteria  in 
[Murry 2002] are satisfied.  This is done by returning the trial elastic stress state back to 
the  yield  surface.    The  stress  and  strain  tensors  are  partitioned  into  elastic  and  plastic 
parts.  Partitioning is done with a return mapping algorithm which enforces the plastic 
consistency condition.  
Separate plasticity algorithms are formulated for the parallel and perpendicular 
modes by enforcing  separate consistency conditions.  The solution  of each  consistency 
condition  determines  the  consistency  parameters,    and  .    The  Δλ  solutions,  in 
turn, determine the stress updates.  No input parameters are required. 
The  stresses  are  readily  updated  from  the  total  strain  increments  and  the 
consistency parameters, as follows: 
𝑛+1 =   𝜎𝑖𝑗
𝜎̅̅̅̅̅𝑖𝑗
∗𝑛+1 − 𝐶𝑖𝑗𝑘𝑙Δ𝜆
𝜕𝑓
𝜕𝜎𝑘𝑙
∣
∗𝑛+1 = 𝜎𝑖𝑗
𝜎𝑖𝑗
𝑛 + 𝐶𝑖𝑗𝑘𝑙Δ𝜀𝑘𝑙
(22.105.6)
(22.105.7)
LS-DYNA Theory Manual 
Material Models 
∗are the trial elastic 
Here 𝑛 denotes the nth time step in the finite element analysis, and 𝜎𝑖𝑗
stress  updates  calculated  from  the  total  strain  increments,  Δ𝜀𝑖𝑗,  prior  to  application  of 
plasticity.  Each normal stress update depends on the consistency parameters and yield 
surface  functions  for  both  the  parallel  (= ||  and  𝑓 = 𝑓||)  and  perpendicular  (=
 and  𝑓 = 𝑓)  modes.    Each  shear  stress  update  depends  on  just  one  consistency 
parameter  and  yield  surface  function.    If  neither  parallel  nor  perpendicular  yielding 
occurs (𝑓||
∗ < 0) then = 0 and the stress update is trivial: 𝜎̂𝑖𝑗
∗ < 0 and 𝑓⊥
𝑛+1 = 𝜎𝑖𝑗
∗𝑛+1. 
Wood exhibits pre-peak nonlinearity in compression parallel and perpendicular 
to  the  grain.    Separate  translating  yield  surface  formulations  are  modeled  for  the 
parallel  and  perpendicular  modes,  which  simulate  gradual  changes  in  moduli.    Each 
initial yield surface hardens until it coincides with the ultimate yield surface.  The initial 
location  of  the  yield  surface  determines  the  onset  of  plasticity.    The  rate  of  translation 
determines the extent of the nonlinearity. 
For each mode (parallel and perpendicular), the user inputs two parameters: the 
initial  yield  surface  location  in  uniaxial  compression,  𝑁,  and  the  rate  of  translation,  𝑐.  
Say  the  user  wants  pre-peak  nonlinearity  to  initiate  at  70%  of  the  peak  strength.    The 
user will input 𝑁 = 0.3 so that 1 − 𝑁 = 0.7.  If the user wants to harden rapidly, then a 
large value of 𝑐 is input, like 𝑐 = 1 msec.  If the user wants to harden gradually, then a 
small value of 𝑐 is input, like 𝑐 = 0.2 msec.  
The state variable that defines the translation of the yield surface is known as the 
back stress, and is denoted by 𝑖𝑗.  Hardening is modeled in compression, but not shear, 
so  the  only  back  stress  required  for  the  parallel  modes  is 11.    The  value  of  the  back 
stress  is  11 = 0  upon  initial  yield  and  11 = −𝑁|| 𝑋𝑐  at  ultimate  yield  (in  uniaxial 
compression).    The  maximum  back  stress  occurs  at  ultimate  yield  and  is  equal  to  the 
total  translation  of  the  yield  surface  in  stress  space.    The  back  stress  components 
required for the perpendicular modes are 22 and 33.  The value of the backstress sum 
XT
Tension
-(1-NII)Xc
-xc
Initial Yield Surface
Ultimate Yield Surace
Compression
SII
Square root of parallel shear invariant
Xc
(1-NII)Xc
|
|
Ultimate Yield Strength
CII large
CII small
Increasing Rate of Translation
NIIXc
Initial Yield Strength
Strain
(a) Initial and ultimate yield surfaces 
(b) Stress-strain behavior 
Figure 22.105.2.  Pre-peak nonlinearity in compression is modeled with
translating yield surfaces that allow the user to specify the hardening response.
Material Models 
LS-DYNA Theory Manual 
is  22 + 33 = 0  upon  initial  yield  and  22 + 33 = −𝑁 𝑌𝑐  at  ultimate  yield  (biaxial 
compression without shear). 
Separate  damage  formulations  are  modeled  for  the  parallel  and  perpendicular 
modes.    These  formulations  are  loosely  based  on  the  work  of  Simo  and  Ju  [1987].    If 
failure  occurs  in  the  parallel  modes,  then  all  six  stress  components  are  degraded 
uniformly.    This  is  because  parallel  failure  is  catastrophic,  and  will  render  the  wood 
useless.  If failure occurs in the perpendicular modes, then only the perpendicular stress 
components are degraded.  This is because perpendicular failure is not catastrophic: we 
expect  the  wood  to  continue  to  carry  load  in  the  parallel  direction.    Based  on  these 
assumptions, the following degradation model is implemented:  
𝑑m =   max(𝑑(𝜏||), 𝑑(𝜏⊥)) ,
𝑑|| = 𝑑(𝜏||), 
𝜎11 = (1 − 𝑑||)𝜎̅̅̅̅̅11, 
𝜎22 = (1 − 𝑑m)𝜎̅̅̅̅̅22, 
𝜎33 = (1 − 𝑑m)𝜎̅̅̅̅̅33, 
σ12 = (1 − 𝑑||)𝜎̅̅̅̅̅12, 
𝜎13 = (1 − 𝑑||)𝜎̅̅̅̅̅13, 
𝜎23 = (1 − 𝑑m)𝜎̅̅̅̅̅23.
(22.105.8)
Here, each scalar damage parameter, 𝑑, transforms the stress tensor associated with the 
undamaged state, 𝜎̅̅̅̅̅𝑖𝑗, into the stress tensor associated with the damaged state, 𝑖𝑗. The 
stress  tensor  𝜎̅̅̅̅̅𝑖𝑗  is  calculated  by  the  plasticity  algorithm  prior  to  application  of  the 
damage  model.    Each  damage  parameter  ranges  from  zero  for  no  damage  and 
approaches  unity  for  maximum  damage.    Thus  1 − 𝑑  is  a  reduction  factor  associated 
with the amount of damage.  Each damage parameter evolves as a function of a strain 
energy-type  term.    Mesh  size  dependency  is  regulated  via  a  length  scale  based  on  the 
element  size  (cube  root  of  volume).    Damage-based  softening  is  brittle  in  tension,  less 
brittle  in  shear,  and  ductile  (no  softening)  in  compression,  as  demonstrated  in  Figure 
22.105.1. 
Element  erosion  occurs  when  an  element  fails  in  the  parallel  mode,  and  the 
parallel  damage  parameter  exceeds  𝑑|| = 0.99.      Elements  do  not  automatically  erode 
when an element fails in the perpendicular mode.  A flag is available, which, when set, 
allows elements to erode when the perpendicular damage parameter exceeds 𝑑 = 0.99. 
Setting this flag is not recommended unless excessive perpendicular damage is causing 
computational difficulties.
LS-DYNA Theory Manual 
Material Models 
(a) Tensile softening. 
(b) Shear softening. 
(c) Compressive yielding. 
Figure 19.143.3.  Softening response modeled for parallel modes of Southern yellow 
pine. 
Data  available  in  the  literature  for  pine  [Reid  &  Peng,  1997]  indicates  that 
dynamic strength enhancement is more pronounced in the perpendicular direction than 
in  the  parallel  direction.    Therefore,  separate  rate  effects  formulations  are  modeled  for
Material Models 
LS-DYNA Theory Manual 
the  parallel  and  perpendicular  modes.    The  formulations  increase  strength  with 
increasing strain rate by expanding each yield surface:   
𝜎11 =  𝑋 + 𝐸11𝜀̇ 𝜂||
𝜎22 = 𝑌 + 𝐸22𝜀̇ 𝜂⊥
Parallel
Perpendicular
.
(22.105.9)
Here  𝑋  and  𝑌  are  the  static  strengths,  11  and  22  are  the  dynamic  strengths,  and 
𝐸11𝜀̇ 𝜂||  and  𝐸22𝜀̇ 𝜂⊥  are  the  excess  stress  components.    The  excess  stress  components 
depend on the value of the fluidity parameter, , as well as the stiffness and strain rate.  
The user inputs two values, 0 and 𝑛, to define each fluidity parameter: 
𝜂|| =
𝜂⊥ =
𝜂0||
𝜀̇𝑛||
𝜂0⊥
𝜀̇𝑛⊥
,
.
(22.105.10)
The  two  parameter  formulation  [Murray,  1997]  allows  the  user  to  model  a 
nonlinear variation in dynamic strength with strain rate.  Setting 𝑛 = 0 allows the user 
to model a linear variation in dynamic strength with strain rate.
LS-DYNA Theory Manual 
Material Models 
22.106  Material Model 144:  Pitzer Crushable Foam 
The logarithmic volumetric strain is defined in terms of the relative volume, 𝑉, as: 
In defining the curves the stress and strain pairs should be positive values starting with 
a volumetric strain value of zero. 
𝛾 = −ln(𝑉).
(22.106.1)
Viscous  damping in the model follows an implementation identical to that of material 
type 57.
Material Models 
LS-DYNA Theory Manual 
22.107  Material Model 147:  FHWA Soil Model 
A brief discussion of the FHWA soil model is given.  The elastic properties of the 
soil are isotropic.  The implementation of the modified Mohr-Coulomb plasticity surface 
is based on the work of Abbo and Sloan [1995].  The model is extended to include excess 
pore water effects, strain softening, kinematic hardening, strain rate effects, and element 
deletion.  
The  modified  yield  surface  is  a  hyperbola  fitted  to  the  Mohr-Coulomb  surface.  
At  the  crossing  of  the  pressure  axis  (zero  shear  strength)  the  modified  surface  is  a 
smooth surface and it is perpendicular to the pressure axis.  The yield surface is given 
as  
𝐹 = −𝑃sin𝜙 + √𝐽2𝐾(𝜃)2 + AHYP2sin2𝜙 − 𝑐cos𝜙 = 0,
(22.107.1)
where 𝑃 is the pressure, 𝜙 is the internal friction angle, 𝐾(𝜃) is a function of the angle in 
𝐹 = −𝑃sin𝜑 + √𝐽2𝐾(𝜃)2 + AHYP2sin2𝜑 − 𝑐cos𝜑 = 0,
(22.107.2)
deviatoric plane, √𝐽2 is the square root of the second invariant of the stress deviator, 𝑐 is 
the amount of cohesion and  
, 
cos3𝜃 =
3√3𝐽3
2𝐽2
J3 is the third invariant of the stress deviator, AHYP is a parameter for determining how 
close to the standard Mohr-Coulomb yield surface the modified surface is fitted.  If the 
user defined parameter, AHYP, is input as zero, the standard Mohr-Coulomb surface is 
recovered.    The  parameter  aℎypshould  be  set  close  to  zero,  based  on  numerical 
considerations, but always less than 𝑐 cot𝜙.  It is best not to set the cohesion, 𝑐, to very 
small values as this causes excessive iterations in the plasticity routines.  
(22.107.3)
To  generalize  the  shape  in  the  deviatoric  plane,  we  have  changed  the  standard 
Mohr- Coulomb 𝐾(𝜃) function to a function used by Klisinski [1985] 
𝐾(𝜃) =
4(1 − 𝑒2)cos2𝜃 + (2𝑒 − 1)2
2(1 − 𝑒2)cos𝜃 + (2𝑒 − 1)[4(1 − 𝑒2)cos2𝜃 + 5𝑒2 − 4𝑒]
, 
(22.107.4)
where  𝑒  is  a  material  parameter  describing  the  ratio  of  triaxial  extension  strength  to 
triaxial  compression  strength.    If  e  is  set  equal  to  1,  then  a  circular  cone  surface  is 
formed.  If 𝑒 is  set to 0.55, then a triangular surface is  found, 𝐾(𝜃) is defined for 0.5 <
𝑒 ≤ 1.0.
LS-DYNA Theory Manual 
Material Models 
Figure 22.107.1.  Pressure versus volumetric strain showing the effects of D1
parameter. 
To  simulate  non-linear  strain  hardening  behavior  the  friction,  angle  𝜙  is 
increased as a function of the effective plastic strain,  
Δ𝜑 = 𝐸t (1 −
𝜑 − 𝜑init
𝐴𝑛𝜑max
) Δ𝜀eff plas.
(22.107.5)
where  𝜀eff  plas  is  the  effective  plastic  strain.  𝐴𝑛  is  the  fraction  of  the  peak  strength 
internal  friction  angle  where  nonlinear  behavior  begins,  0 < 𝐴𝑛 ≤ 1.    The  input 
parameter 𝐸𝑡 determines the rate of the nonlinear hardening.  
To  simulate  the  effects  of  moisture  and  air  voids  including  excess  pore  water 
pressure, both the elastic and plastic behaviors can be modified.  The bulk modulus is   
𝐾 =
𝐾𝑖
1 + 𝐾𝑖𝐷1𝑛cur
.
(22.107.6)
where  
𝐾𝑖 = initial bulk modulus 
𝑛cur = current porosity  =  Max[0, (𝑤 − 𝜀v)] 
𝑤 = volumetric strain corresponding to the volume of air voids  = 𝑛(1 − 𝑆) 
𝜀v = total volumetric strain 
𝐷1 = material constant controlling the stiffness before the air voids are collapsed 
𝑛 = porosity of the soil  =  
1 + 𝑒
Material Models 
LS-DYNA Theory Manual 
Figure 22.107.2.  The effect on pressure due to pore water pressure. 
𝑒 = void ratio  =  
γsp(1 + mc)
− 1 
𝑆 = degree of saturation  =  
𝜌𝑚c
𝑛(1 + 𝑚c)
and 𝜌, 𝛾, 𝑚c are the soil density, specific gravity, and moisture content, respectively. 
Figure 22.107.1 shows the effect of the 𝐷1 parameter on the pressure-volumetric 
strain relationship (bulk modulus).  The bulk modulus will always be a monotonically 
increasing value, i.e.,  
𝐾𝑗+1 =
𝐾𝑖
1 + 𝐾𝑖𝐷1𝑛cur
𝐾𝑗
⎧
{
⎨
{
⎩
if 𝜀𝑣 𝑗+1 > 𝜀𝑣𝑗
. 
if 𝜀𝑣 𝑗+1 ≤ 𝜀𝑣𝑗
(22.107.7)
Note that the model is following the standard practice of assuming compressive 
stresses  and  strains  are  positive.    If  the  input  parameter  𝐷1  is  zero,  then  the  standard 
linear elastic bulk modulus behavior is used. 
To simulate the loss of shear strength due to excess pore water effects, the model 
uses a standard soil mechanics technique [Holtz and Kovacs, 1981] of reducing the total 
pressure,  𝑃,  by  the  excess  pore  water  pressure,  𝑢,  to  get  an  “  effective  pressure”,  𝑃′; 
therefore, 
𝑃′ = 𝑃 − 𝑢.
(22.107.8)
Figure  22.107.2  shows  pore  water  pressure  will  affect  the  algorithm  for  the 
plasticity surface.  The excess pore water pressure reduces the total pressure, which will
LS-DYNA Theory Manual 
Material Models 
lower the shear strength, √𝐽2.  A large excess pore water pressure can cause the effective 
pressure to become zero. 
To calculate the pore water pressure, 𝑢, the model uses an equation similar to the 
equation used for the moisture effects on the bulk modulus. 
𝑢 =
𝐾sk
1 + 𝐾sk𝐷2𝑛cur
𝜀𝑣,
(22.107.9)
where  
𝐾sk = bulk modulus for soil without air voids (skeletal bulk modulus) 
𝑛cur = current porosity  =  Max[0, (𝑤 − 𝜀𝑣)] 
𝑤 = volumetric strain corresponding to the volume of air voids  = 𝑛(1 − 𝑆) 
𝜀v = total volumetric strain 
𝐷2 = material constant controlling the pore water pressure before  
             the air voids are collapsed to 𝐷2 ≥ 0 
𝑛 = porosity of the soil =
𝑒 = void ratio  =  
1 + 𝑒
γsp(1 + mc)
𝑆 = degree of saturation  =  
− 1 
𝜌𝑚c
𝑛(1 + 𝑚c)
and  𝜌,  𝛾,  𝑚c  are  the  soil  density,  specific  gravity,  and  moisture  content,  respectively.  
The pore water pressure will not be allowed to become negative, 𝑢 ≥ 0.  
Figure 22.107.3 is a plot of the pore pressure versus volumetric strain for different 
parameter  values.    With  the 𝐷2  parameter  set relatively  high  compared  to 𝐾sk  there  is 
no  pore  pressure  until  the volumetric  strain is  greater than  the  strains  associated  with 
the air voids.  However, as 𝐷2 is lowered, the pore pressure starts to increase before the 
air  voids  are  totally  collapsed.    The  𝐾sk  parameter  affects  the  slope  of  the  post-void 
collapse pressure - volumetric behavior.
Material Models 
LS-DYNA Theory Manual 
The parameter 𝐷2 can  be found from Skempton pore water pressure parameter 
𝐵, where 𝐵 is defined as [Holtz and Kovacs, 1981]: 
𝐵 =
𝐷2 =
,
1 + 𝑛
𝐾sk
𝐾v
1 − 𝐵
𝐵𝐾sk[𝑛(1 − 𝑆)]
.
(22.107.10)
To  simulate  strain  softening  behavior  the  FHWA  soil  model  uses  a  continuum 
damage algorithm.  The strain-based damage algorithm is based on the work of J. W. Ju 
and  J.  C.  Simo  [1987,  1989].    They  proposed  a  strain  based  damage  criterion,  which  is 
uncoupled from the plasticity algorithm.   
For the damage criterion,  
𝜉 = −
𝐾𝑖
∫ 𝑃̅̅̅̅̅𝑑𝜀pv,
(22.107.11)
where 𝑃̅̅̅̅̅  is  the  pressure  and  𝜀pv  is  the  plastic  volumetric  strain,  the  damaged  stress  is 
found from the undamaged stresses.  
𝜎 = (1 − 𝑑)𝜎̅̅̅̅̅,
(22.107.12)
where 𝑑 is the isotropic damage parameter.  The damage parameter is found at step 𝑗 +
1 as: 
 Figure 22.107.3.  The effects of 𝐷2 and 𝐾sk parameters on pore water pressure.
LS-DYNA Theory Manual 
Material Models 
𝑑𝑗+1 = 𝑑𝑗   
if
𝜉𝑗+1 ≤ 𝑟𝑗
𝑑𝑗+1 =
𝜉𝑗+1 − 𝜉0
𝛼 − 𝜉0
if
𝜉𝑗+1 > 𝑟𝑗
, 
(22.107.13)
where  𝑟t  is  a  damage  threshold  surface,  𝑟𝑗+1 = max{𝑟𝑗, 𝜉𝑗+1),  and  𝜉0 = 𝑟0  (DINT).    The 
mesh sensitivity parameter, 𝛼, will be described below. 
Typically, the damage, 𝑑, varies from 0 to a maximum of 1.  However, some soils 
can  have  a  residual  strength  that  is  pressure  dependent.    The  residual  strength  is 
represented by 𝜙res, the minimum internal friction angle. 
The maximum damage allowed is related to the internal friction angle of residual 
strength by: 
𝑑max =
sin𝜙 − sin𝜙res
sin𝜙
,
(22.107.14)
If  𝜙res > 0,  then  𝑑max,  the  maximum  damage,  will  not  reach  1,  and  the  soil  will  have 
some residual strength. 
When material models include strain softening, special techniques must be used 
to  prevent  mesh  sensitivity.    Mesh  sensitivity  is  the  tendency  of  the  finite  element 
model/analysis to produce significantly different results as the element size is reduced.  
The  mesh  sensitivity  occurs  because  the  softening  in  the  model  concentrates  in  one 
element.    As  the  element  size  is  reduced  the  failure  becomes  localized  in  smaller 
volumes,  which  causes  less  energy  to  be  dissipated  by  the  softening  leading  to 
instabilities or at least mesh sensitive behavior.  
To  eliminate  or  reduce  the  effects  of  strain  softening  mesh  sensitivity,  the 
softening parameter, α (the strain at full damage), must be modified as the element size 
changes.   The FHWA soil model uses an input parameter, “void formation”, 𝐺f, that is 
like fracture energy material property for metals.  The void formation parameter is the 
area under the softening region of the pressure volumetric strain curve times the cube 
root of the element volume, 𝑉
3.   
𝐺f = 𝑉
3 ∫ 𝑃
𝜉0
𝑑𝜀v =
𝑃peak(𝛼 − 𝜉0)𝑉
,
(22.107.15)
with 𝜉0, the volumetric strain at peak pressure (strain at initial damage, DINT).  Then 𝛼 
can be found as a function of the volume of the element 𝑉: 
𝛼 =
2𝐺f
3⁄
𝐾𝜉0𝑉
+ 𝜉0.
(22.107.16)
Material Models 
LS-DYNA Theory Manual 
If 𝐺f is made very small relative to 𝐾𝜉0𝑉
3⁄ , then the softening behavior will be 
brittle.  
Strain-rate  enhanced  strength 
is  simulated  by  a  two-parameter  Devaut-Lions 
viscoplastic update algorithm, developed by Murray [1997].  This algorithm interpolates 
between  the  elastic  trial  stress  (beyond  the  plasticity  surface)  and  the  inviscid  stress.  
The inviscid stresses (𝜎̅̅̅̅̅) are on the plasticity surface.   
Δ𝑡+𝜂, and 𝜂 = (
𝜎̅̅̅̅̅vp = (1 − 𝜍)𝜎̅̅̅̅̅ + 𝜍𝜎̅̅̅̅̅trial,
𝛾r
𝜀̇ )(𝑣𝑛−1)/𝑣𝑛. 
where 𝜍 =
(22.107.17)
As  𝜁   approaches  1,  then  the  viscoplastic  stress  becomes  the  elastic  trial  stress.  
Setting the input value 𝛾r = 0 eliminates any strain-rate enhanced strength effects.  
The model allows element deletion, if needed.  As the strain softening  (damage) 
increases,  the  effective  stiffness  of  the  element  can  get  very  small,  causing  severe 
element  distortion  and  hourglassing.    The  element  can  be  “deleted”  to  remedy  this 
behavior.    There  are  two  input  parameters  that  affect  the  point  of  element  deletion.  
DAMLEV  is  the  damage  threshold  where  element  deletion  will  be  considered.  
EPSPRMAX is the maximum principal strain where element will be deleted.  Therefore, 
𝑑 ≥ DAMLEV    and 𝜀prmax > EPSPRMAX,
(22.107.18)
for element deletion to occur.  If DAMLEV  is set to zero, there is no element deletion.  
Care must be taken when employing element deletion to assure that the internal forces 
are very small (element stiffness is zero) or significant errors can be introduced into the 
analysis.  
The keyword option, NEBRASKA, gives the soil parameters used to validate the 
material model with experiments performed at University of Nebraska at Lincoln.  The 
units for this default inputs are milliseconds, kilograms, and millimeters.  There are no 
required  input  parameters  except  material  id  (MID).    If  different  units  are  desired  the 
unit conversion factors that need to multiply the default parameters can be input.
LS-DYNA Theory Manual 
Material Models 
22.108  Material Model 154:  Deshpande-Fleck Foam 
The equivalent stress, 𝜎̂ , is given by: 
𝛷 = 𝜎̂ − 𝜎Y,
𝜎̂ 2 =
2 + 𝛼2𝜎m
𝜎VM
1 + (𝛼/3)2 ,
where, 𝜎VM, is the von Mises effective stress, 
𝜎VM = √
𝛔dev: 𝛔dev,
and, 𝜎mand 𝛔dev, is the mean and deviatoric stress 
𝜎m = tr(𝛔)
𝛔dev = 𝛔 − σm𝐈.
The yield stress 𝜎Y can be expressed as 
𝜎Y = 𝜎p + 𝛾
𝜀̂
𝜀D
+ 𝛼2 (
1 − (𝜀̂/𝜀D)𝛽
),
(22.108.1)
(22.108.2)
(22.108.3)
(22.108.4)
(22.108.5)
Here, 𝜎p, 𝛼2, 𝛾 and 𝛽 are material parameters.  The densification strain, 𝜀D, is defined as 
𝜌f
𝜌f0
𝜀D = −ln (
(22.108.6)
),
where 𝜌f is the foam density and 𝜌f0 is the density of the virgin material.
Material Models 
LS-DYNA Theory Manual 
22.109  Material Model 156:  Muscle  
The  material  behavior  of 
from 
*MAT_SPRING_MUSCLE,  the  spring  muscle  model  and  treated  here  as  a  standard 
material.    The  initial  length  of  muscle  is  calculated  automatically.    The  force,  relative 
length  and  shortening  velocity  are  replaced  by  stress,  strain  and  strain  rate.    A  new 
parallel damping element is added. 
the  muscle  model 
adapted 
is 
The strain and normalized strain rate are defined respectively as 
− 1 = 𝐿 − 1 
𝑙𝑜
𝜀 =
𝜀̇ =
𝑙 ̇
𝑙o  𝜀̇max
=
𝑉M
𝑙𝑜 ∗ (SRM ∗ SFR)
=
𝑉M
(𝑙𝑜 ∗ SRM) ∗ SFR
=
𝑉M
𝑉max ∗ SFR
= 𝑉, 
(22.109.1)
where 𝑙𝑜 is the original muscle length. 
From the relation above, it is known: 
𝑙𝑜 =
𝑙0
1 + 𝜀0
,
(22.109.2)
where 𝜀0 = SNO; 𝑙0 = muscle length at time 0.  Stress of Contractile Element is: 
𝜎1 = 𝜎max 𝑎(𝑡)𝑓 (𝜀) 𝑔(𝜀̇),
(22.109.3)
where 𝜎max =PIS; 𝑎(𝑡) =ALM; 𝑓 (𝜀) =SVS; 𝑔(𝜀̇) =SVR.  Stress of Passive Element is: 
𝜎2 = 𝜎maxℎ(ε).
(22.109.4)
For exponential relationship:  
ℎ(ε) =
⎧
{{{{{
{{{{{
⎨
⎩
𝜀 ≤ 0
exp(𝑐) − 1
[ exp (
𝑐𝜀
𝐿max
) − 1 ]
𝜀 > 0    𝑐 ≠ 0
(22.109.5)
⁄
𝜀 𝐿max
𝜀 > 0
𝑐 = 0
where 𝐿max = 1 + SSM; and 𝑐 =CER.  Stress of Damping Element is: 
Total Stress is: 
𝜎3 = 𝐷𝜀̇max𝜀̇
𝜎 = 𝜎1 + 𝜎2 + 𝜎3.
(22.109.6)
(22.109.7)
LS-DYNA Theory Manual 
Material Models 
22.110  Material Model 158:  Rate Sensitive Composite Fabric 
See  material  type  58,  Laminated  Composite  Fabric,  for  the  treatment  of  the 
composite material. 
Rate  effects  are  taken  into  account  through  a  Maxwell  model  using  linear 
viscoelasticity by a convolution integral of the form: 
𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)
𝜕𝜀𝑘𝑙
𝜕𝜏
𝑑𝜏
,
(22.110.1)
where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) is the relaxation function for different stress measures.  This stress is 
added to the stress tensor determined from the strain energy functional.  Since we wish 
to  include  only  simple  rate  effects,  the  relaxation  function  is  represented  by  six  terms 
from the Prony series: 
𝑔(𝑡) = ∑ 𝐺𝑚𝑒−𝛽𝑚𝑡
𝑚=1
.
(22.110.2)
We  characterize  this  in  the  input  by  the  shear  moduli,  𝐺𝑖,  and  the  decay 
constants,  𝛽𝑖.    An  arbitrary  number  of  terms,  not  exceeding  6,  may  be  used  when 
applying  the  viscoelastic  model.    The  composite  failure  is  not  directly  affected  by  the 
presence of the viscous stress tensor.
Material Models 
LS-DYNA Theory Manual 
22.111  Material Model 159:  Continuous Surface Cap Model 
This  is  a  cap  model  with  a  smooth  intersection  between  the  shear  yield  surface 
and hardening cap, as shown in Figure 22.111.1.   The initial damage surface coincides 
with the yield surface.  Rate effects are modeled with viscoplasticity.  See [Murray 2007] 
for a more complete description of the material model. 
Stress Invariants. The yield surface is formulated in terms of three stress invariants: 𝐽1 
is  the  first  invariant  of  the  stress  tensor,  𝐽′2  is  the  second  invariant  of  the  deviatoric 
stress tensor, and 𝐽′3 is the third invariant of the deviatoric stress tensor.  The invariants 
are defined in terms of the deviatoric stress tensor, 𝑆𝑖𝑗 and pressure, 𝑃, as follows: 
𝐽1 = 3𝑃,
𝐽′
2 =
𝑆𝑖𝑗𝑆𝑖𝑗, 
𝐽′
3 =
𝑆𝑖𝑗𝑆𝑗𝑘𝑆𝑘𝑖.
(22.111.1)
Plasticity Surface.  The three invariant yield function is based on these three invariants, 
and the cap hardening parameter, 𝑘, as follows: 
𝑓 (𝐽1, 𝐽′2, 𝐽′3, 𝜅) = 𝐽′2 − ℜ2𝐹f
(22.111.2)
Here 𝐹f is the shear failure surface,  𝐹c is the hardening cap, and ℜ is the Rubin three-
invariant reduction factor.  The cap hardening parameter 𝜅 is the value of the pressure 
invariant at the intersection of the cap and shear surfaces.  
2𝐹c.
Trial  elastic  stress  invariants  are  temporarily  updated  via  the  trial  elastic  stress 
′𝑇.    Elastic  stress  states  are  modeled  when 
tensor,  𝜎 T.  These  are  denoted  𝐽1
′𝑇  and  𝐽3
𝑇  ,  𝐽2
Figure  22.111.1.    General  Shape  of  the  concrete  model  yield  surface  in  two-
dimensions.
LS-DYNA Theory Manual 
Material Models 
 𝑓 (𝐽1, 𝐽′2, 𝐽′3, 𝜅𝑇) < 0.  Elastic-plastic stress states are modeled when 𝑓 (𝐽1, 𝐽′2, 𝐽′3, 𝜅𝑇) > 0.  
In this case, the plasticity algorithm returns the stress state to the yield surface such that 
𝑃, 𝜅𝑃) = 0.    This  is  accomplished  by  enforcing  the  plastic  consistency 
𝑓 (𝐽1
condition with associated flow. 
𝑃, 𝐽′3
𝑃, 𝐽′2
Shear Failure Surface.  The strength of concrete is modeled by the shear surface in the 
tensile and low confining pressure regimes: 
𝐹f(𝐽1) = 𝛼 − 𝜆𝑒−𝛽𝐽1 + 𝜃𝐽1.
(22.111.3)
Here  the  values  of  𝛼,  𝛽,  𝜆,  and  𝜃  are  selected  by  fitting  the  model  surface  to  strength 
measurements  from  triaxial  compression  (txc)  tests  conducted  on  plain  concrete 
cylinders.  
′   (principal  stress 
Rubin  Scaling  Function.    Concrete  fails  at  lower  values  of  √3𝐽2
difference)  for  triaxial  extension  (txe)  and  torsion  (tor)  tests  than  it  does  for  txc  tests 
conducted at the same pressure.  The Rubin scaling function ℜ determines the strength 
of  concrete  for  any  state  of  stress  relative  to the  strength  for  txc,  via  ℜ𝐹𝑓 .    Strength  in 
torsion is modeled as 𝑄1𝐹f.  Strength in txe is modeled as 𝑄2𝐹f, where: 
𝑄1 = 𝛼1 − 𝜆1𝑒−𝛽1𝐽1 + 𝜃1𝐽1,
𝑄2 = 𝛼2 − 𝜆2𝑒−𝛽2𝐽1 + 𝜃2𝐽1.
(22.111.4)
Cap  Hardening  Surface.  The  strength  of  concrete  is  modeled  by  a  combination  of  the 
cap and shear surfaces in the low to high confining pressure regimes.  The cap is used to 
model  plastic  volume  change  related  to  pore  collapse  (although  the  pores  are  not 
explicitly  modeled).      The  isotropic  hardening  cap  is  a  two-part  function  that  is  either 
unity or an ellipse: 
𝐹c( 𝐽1, 𝜅 ) = 1 −
[𝐽1 − 𝐿 (𝜅)][|𝐽1 − 𝐿(𝜅)| + 𝐽1 − 𝐿(𝜅)]
2[𝑋(𝜅) − 𝐿 (𝜅)] 2
,
(22.111.5)
where 𝐿(𝜅) is defined as: 
L(κ) = {
if
𝜅 > 𝜅0
𝜅0 otherwise
.
(22.111.6)
The equation for 𝐹c is equal to unity for 𝐽1  𝐿(𝜅).  It describes the ellipse for 𝐽1 >
𝐿(𝜅). The intersection of the shear surface and the cap is at 𝐽1 = 𝜅.  𝜅0 is the value of 𝐽1 at 
the initial intersection of the cap and shear surfaces before hardening is engaged (before 
the cap moves).  The  equation for 𝐿(𝜅) restrains the cap from retracting past its initial 
location at 𝜅0.   
The  intersection  of  the  cap  with  the  𝐽1  axis  is  at  𝐽1 = 𝑋(𝜅).    This  intersection 
depends upon the cap ellipticity ratio 𝑅, where 𝑅 is the ratio of its major to minor axes: 
𝑋(𝜅) = 𝐿(𝜅) + 𝑅𝐹f(𝐿(𝜅)).
(22.111.7)
Material Models 
LS-DYNA Theory Manual 
  The  cap  expands  (𝑋(𝜅) 
The  cap  moves  to  simulate  plastic  volume  change. 
and 𝜅  increase) to simulate plastic volume compaction.  The cap contracts (𝑋(𝜅) and 𝜅 
decrease) to simulate plastic volume expansion, called dilation.  The motion (expansion 
and contraction) of the cap is based upon the hardening rule:  
p = 𝑊(1 − 𝑒−𝐷1(𝑋−𝑋0)−𝐷2(𝑋−𝑋0)2
𝜀𝑣
(22.111.8)
p the plastic volume strain, 𝑊 is the maximum plastic volume strain, and 𝐷1 and 
Here 𝜀v
𝐷2 are model input parameters.  𝑋0 is the initial location of the cap when 𝜅 = 𝜅0. 
).
The  five  input  parameters  (𝑋0,  𝑊,  𝐷1,  𝐷2,  and  𝑅)  are  obtained  from  fits  to  the 
pressure-volumetric  strain  curves  in  isotropic  compression  and  uniaxial  strain.  𝑋0 
determines  the  pressure  at  which  compaction  initiates  in  isotropic  compression.  𝑅 
combined  with  𝑋0,  determines  the  pressure  at  which  compaction  initiates  in  uniaxial 
strain.  𝐷1  and  𝐷2  determine  the  shape  of  the  pressure-volumetric  strain  curves.    𝑊 
determines the maximum plastic volume compaction. 
Shear  Hardening  Surface.    In  unconfined  compression,  the  stress-strain  behavior  of 
concrete  exhibits  nonlinearity  and  dilation  prior  to  the  peak.    Such  behavior  is  be 
modeled with an initial shear yield surface, 𝑁H𝐹f, which hardens until it coincides with 
the  ultimate  shear  yield  surface,  𝐹f.    Two  input  parameters  are  required.    One 
parameter, 𝑁H, initiates hardening by setting the location of the initial yield surface.  A 
second parameter, 𝐶H, determines the rate of hardening (amount of nonlinearity). 
Damage.    Concrete  exhibits  softening  in  the  tensile  and  low  to  moderate  compressive 
regimes. 
𝑑 = (1 − 𝑑)𝜎𝑖𝑗
𝜎𝑖𝑗
vp,
(22.111.9)
A  scalar  damage  parameter,  𝑑,  transforms  the  viscoplastic  stress  tensor  without 
damage,  denoted  𝜎 vp,  into  the  stress  tensor  with  damage,  denoted  𝜎 d.    Damage 
accumulation  is  based  upon  two  distinct  formulations,  which  we  call  brittle  damage 
and ductile damage.  The initial damage threshold is coincident with the shear plasticity 
surface, so the threshold does not have to be specified by the user.   
Ductile  Damage.      Ductile  damage  accumulates  when  the  pressure  (𝑃)  is  compressive 
and  an  energy-type  term,  𝜏c,  exceeds  the  damage  threshold,  𝜏0c.    Ductile  damage 
accumulation depends upon the total strain components, 𝜀𝑖𝑗, as follows:  
𝜏c = √
𝜎𝑖𝑗𝜀𝑖𝑗
(22.111.10)
The  stress  components  𝜎𝑖𝑗  are  the  elasto-plastic  stresses  (with  kinematic  hardening) 
calculated before application of damage and rate effects.
LS-DYNA Theory Manual 
Material Models 
Brittle  Damage.    Brittle  damage  accumulates  when  the  pressure  is  tensile  and  an 
energy-type term, 𝜏t, exceeds the damage threshold, 𝜏0t.  Brittle damage accumulation 
depends upon the maximum principal strain, 𝜀max, as follows: 
𝜏t = √𝐸𝜀max
.
(22.111.11)
Softening Function.  As damage accumulates, the damage parameter 𝑑 increases from 
an  initial  value  of  zero,  towards  a  maximum  value  of  one,  via  the  following 
formulations: 
Brittle Damage: 
𝑑(𝜏1) =
0.999
(
1 + 𝐷
1 + 𝐷exp[−𝐶(𝜏𝑡 − 𝜏0𝑡)]
− 1). 
Ductile Damage: 
𝑑(𝜏1) =
𝑑max
(
1 + 𝐵
1 + 𝐵exp[−𝐴(𝜏c − 𝜏0c)]
− 1). 
(22.111.12)
(22.111.13)
The  damage  parameter  that  is  applied  to  the  six  stresses  is  equal  to  the  current 
maximum of the brittle or ductile damage parameter.  The parameters 𝐴 and 𝐵 or 𝐶 and 
𝐷  set  the  shape  of  the  softening  curve  plotted  as  stress-displacement  or  stress-strain.  
The parameter 𝑑max is the maximum damage level that can be attained.  It is internally 
calculated and is less than one at moderate confining pressures .    The  compressive  softening  parameter,  𝐴,  may  also  be 
reduced with confinement, using the input parameter PMOD, as follows:  
𝐴 = 𝐴(𝑑max + 0.001)PMOD.
(22.111.14)
Regulating  Mesh  Size  Sensitivity.    The  concrete  model  maintains  constant  fracture 
energy,  regardless  of  element  size.    The  fracture  energy  is  defined  here  as  the  area 
under the stress-displacement curve from peak strength to zero strength.  This is done 
by  internally  formulating  the  softening  parameters  𝐴  and  𝐶  in  terms  of  the  element 
length, 𝑙 (cube root of the element volume), the fracture energy, 𝐺f, the initial damage 
threshold, 𝜏0t or 𝜏0c, and the softening shape parameters, 𝐷 or 𝐵. 
The fracture energy is calculated from up to five user-specified input parameters 
(𝐺fc,  𝐺ft,  𝐺fs,  pwrc,  pwrc).    The  user  specifies  three  distinct  fracture  energy  values.  
These  are  the  fracture  energy  in  uniaxial  tensile  stress,  𝐺ft,  pure  shear  stress,  𝐺fs,  and 
uniaxial compressive stress, 𝐺fc.  The model internally selects the fracture energy from 
equations  which  interpolate  between  the  three  fracture  energy  values  as  a  function  of 
the  stress  state  (expressed  via  two  stress  invariants).    The  interpolation  equations 
depend upon the user-specified input powers PWRC and PWRT, as follows. 
if the pressure is tensile 
(22.111.15)
Material Models 
LS-DYNA Theory Manual 
 𝐺f = 𝐺fs + trans(𝐺ft − 𝐺fs)  where trans =
if the pressure is compressive  
PWRT
⎜⎜⎜⎛ −𝐽1
√3𝐽′
⎝
⎟⎟⎟⎞
2⎠
𝐺f = 𝐺fs + trans(𝐺fc − 𝐺fs) where trans =
PWRC
⎜⎜⎜⎛ 𝐽1
⎟⎟⎟⎞
√3𝐽′2⎠
⎝
The internal parameter trans is limited to range between 0 and 1. 
Element  Erosion.    An  element  loses  all  strength  and  stiffness  as  𝑑 → 1.    To  prevent 
computational difficulties with very low stiffness, element erosion is available as a user 
option.  An element erodes when 𝑑 > 0.99 and the maximum principal strain is greater 
than a user supplied input value, 1-erode. 
Viscoplastic  Rate  Effects.    At  each  time  step,  the  viscoplastic  algorithm  interpolates 
p,  to 
between  the  elastic  trial  stress,  𝜎𝑖𝑗
set the viscoplastic stress (with rate effects), 𝜎𝑖𝑗
T,  and  the  inviscid  stress  (without  rate  effects),  𝜎𝑖𝑗
vp:   
vp = (1 − 𝛾)𝜎𝑖𝑗
𝜎𝑖𝑗
p,
T + 𝛾𝜎𝑖𝑗
(22.111.16)
with 𝛾 =
Δ𝑡/𝜂
1+Δ𝑡/𝜂. 
This interpolation depends upon the effective fluidity coefficient, , and the time 
step, 𝑡.  The effective fluidity coefficient is internally calculated from five user-supplied 
input parameters and interpolation equations: 
if the pressure is tensile 
𝜂 = 𝜂s + trans(𝜂t − 𝜂s)          trans =
if the pressure is compressive  
𝜂 = 𝜂s + trans(𝜂c − 𝜂s)          trans =
 𝜂t =
𝜂0t
𝜀̇Nt
     𝜂c =
𝜂0c
𝜀̇Nc
𝜂s = SRATE 𝜂t
pwrt
⎜⎜⎜⎛ −𝐽1
√3𝐽′
⎝
⎟⎟⎟⎞
2⎠
pwrc
⎜⎜⎜⎛ 𝐽1
√3𝐽′
⎝
⎟⎟⎟⎞
2⎠
(22.111.17)
The input parameters are 𝜂0t and 𝑁t for fitting uniaxial tensile stress data, 𝜂0c and 𝑁c for 
fitting the uniaxial compressive stress data, and SRATE for fitting shear stress data.  The 
effective strain rate is 𝜀̇. 
This  viscoplastic  model  may  predict  substantial  rate  effects  at  high  strain  rates 
(𝜀̇ > 100).  To limit rate effects at high strain rates, the user may input overstress limits 
in  tension  (OVERT)  and  compression  (OVERC).    These  input  parameters  limit 
calculation of the fluidity parameter, as follows:
LS-DYNA Theory Manual 
Material Models 
If 𝐸𝜀̇𝜂 > OVER, then = over
𝛦𝜀̇  
(22.111.18)
where  OVER = OVERT  when  the  pressure  is  tensile,  and  OVER = OVERC  when  the 
pressure is compressive. 
The user has the option of increasing the fracture energy as a function of effective 
strain rate via the REPOW input parameter, as follows: 
rate = 𝐺f
𝐺f
⎜⎛1 +
⎝
𝐸𝜀̇𝜂
⎟⎞
𝑟𝑠√𝐸⎠
REPOW
(22.111.19)
rate  is  the  fracture  energy  enhanced  by  rate  effects,  and  𝑟𝑠  is  the  internally 
Here  𝐺f
calculated damage threshold before application of rate effects .  The 
term  in  brackets  is  greater  than,  or  equal  to  one,  and  is  the  approximate  ratio  of  the 
dynamic to static strength.
Material Models 
LS-DYNA Theory Manual 
22.112  Material Models 161 and 162:  Composite MSC 
in 
The  unidirectional  and  fabric  layer  failure  criteria  and  the  associated  property 
degradation models for material 161 are described as follows.  All the failure criteria are 
stresses 
expressed 
(𝜎𝑎, 𝜎𝑏, 𝜎𝑐, 𝜏𝑎𝑏, 𝜏𝑏𝑐, 𝜏𝑐𝑎)  and  the  associated  elastic  moduli  are  (𝐸𝑎, 𝐸𝑏, 𝐸𝑐, 𝐺𝑎𝑏, 𝐺𝑏𝑐, 𝐺𝑐𝑎).  
Note  that  for  the  unidirectional  model, 𝑎,  𝑏  and  𝑐  denote  the  fiber,  in-plane  transverse 
and  out-of-plane  directions,  respectively,  while  for  the  fabric  model,  𝑎,  𝑏  and  𝑐  denote 
the in-plane fill, in-plane warp and out-of-plane directions, respectively.  
components  based  on  ply 
terms  of 
stress 
level 
Unidirectional Lamina Model 
Three criteria are used for fiber failure, one in tension/shear, one in compression 
and another one in crush under pressure.  They are chosen in terms of quadratic stress 
forms as follows: 
Tensile/shear fiber mode:  
𝑓1 = (
)
〈𝜎𝑎〉
𝑆𝑎T
+ (
2 + 𝜏𝑐𝑎
𝜏𝑎𝑏
𝑆FS
) − 1 = 0.
Compression fiber mode: 
𝑓2 = (
′〉
〈𝜎𝑎
𝑆𝑎C
)
− 1  = 0,
′ = −𝜎𝑎 + ⟨−
𝜎𝑎
𝜎𝑏 + 𝜎𝑐
⟩.
Crush mode: 
𝑓3 = (
)
〈𝑝〉
𝑆FC
− 1 = 0,
𝑝 = −
𝜎𝑎 + 𝜎𝑏 + 𝜎𝑐
.
(22.112.1)
(22.112.2)
(22.112.3)
⟩ are Macaulay brackets, 𝑆𝑎T and 𝑆𝑎C are the tensile and compressive strengths 
where ⟨
in the fiber direction, and 𝑆FS and 𝑆FC are the layer strengths associated with the fiber 
shear and crush failure, respectively.  
Matrix mode failures must occur without fiber failure, and hence they will be on 
planes parallel to fibers.  For simplicity, only two failure planes are considered: one is 
perpendicular to the planes of layering and the other one is parallel to them.  The matrix 
failure  criteria  for  the  failure  plane  perpendicular  and  parallel  to  the  layering  planes, 
respectively, have the forms: 
Perpendicular matrix mode: 
𝑓4 = (
)
⟨𝜎𝑏⟩
𝑆𝑏T
+ (
𝜏𝑏𝑐
′ )
𝑆𝑏𝑐
+ (
𝜏𝑎𝑏
𝑆𝑎𝑏
)
− 1 = 0.
Parallel matrix mode (Delamination): 
22-264 (Material Models)
LS-DYNA Theory Manual 
Material Models 
2 
𝑓5 = 𝑆2
{⎧
⎩{⎨
(
⟨𝜎𝑐⟩
𝑆𝑏T
)
+ (
)
𝜏𝑏𝑐
"
𝑆𝑏𝑐
+ (
𝜏𝑐𝑎
𝑆𝑐𝑎
)
}⎫
⎭}⎬
− 1 = 0,
(22.112.5)
where  𝑆𝑏T  is  the  transverse  tensile  strength.    Based  on  the  Coulomb-Mohr  theory,  the 
shear strengths for the transverse shear failure and the two axial shear failure modes are 
assumed to be the forms, 
𝑆𝑎𝑏 = 𝑆𝑎𝑏
′ = 𝑆𝑏𝑐
𝑆𝑏𝑐
𝑆𝑐𝑎 = 𝑆𝑐𝑎
" = 𝑆𝑏𝑐
𝑆𝑏𝑐
(0) + tan(𝜑)⟨−𝜎𝑏⟩,
(0) + tan(𝜑)⟨−𝜎𝑏⟩, 
(0) + tan(𝜑)⟨−𝜎𝑐⟩, 
(0) + tan(𝜑)⟨−𝜎𝑐⟩,
(22.112.6)
where 𝜑 is a material constant as tan(𝜑) is similar to the coefficient of friction, and 𝑆𝑎𝑏
(0)are the shear strength values of the corresponding tensile modes.  
(0) and 𝑆𝑏𝑐
𝑆𝑐𝑎
(0), 
Failure  predicted  by  the  criterion  of  𝑓4  can  be  referred  to  as  transverse  matrix 
failure,  while  the  matrix  failure  predicted  by  𝑓5,  which  is  parallel  to  the  layer,  can  be 
referred as the delamination mode when it occurs within the elements that are adjacent 
to the ply interface.  Note that a scale factor 𝑆 is introduced to provide better correlation 
of delamination area with experiments.  The scale factor 𝑆 can be determined by fitting 
the analytical prediction to experimental data for the delamination area. 
When  fiber  failure  in  tension/shear  mode  is  predicted  in  a  layer  by 𝑓1,  the  load 
carrying capacity of that layer is completely eliminated.  All the stress components are 
reduced  to  zero  instantaneously  (100  time  steps  to  avoid  numerical  instability).    For 
compressive fiber failure, the layer is assumed to carry a residual axial load, while the 
transverse  load  carrying  capacity  is  reduced  to  zero.    When  the  fiber  compressive 
failure mode is reached due to 𝑓2, the axial layer compressive strength stress is assumed 
to  reduce  to  a  residual  value  SRC  (=SFFC ∗ SAC).    The  axial  stress  is  then  assumed  to 
remain  constant,  i.e.,  𝜎𝑎 = −𝑆RC,  for  continuous  compressive  loading,  while  the 
subsequent  unloading  curve  follows  a  reduced  axial  modulus  to  zero  axial  stress  and 
strain  state.    When  the  fiber  crush  failure  occurs,  the  material  is  assumed  to  behave 
elastically for compressive pressure, 𝑝 > 0, and to carry no load for tensile pressure, 𝑝 <
0.  
(0)and 𝑆𝑏𝑐
When  a  matrix  failure  (delamination)  in the a-b  plane  is  predicted,  the  strength 
(0) are set to zero.  This results in reducing the stress components 𝜎𝑐, 
values for 𝑆𝑐𝑎
𝜏𝑏𝑐  and  𝜏𝑐𝑎  to  the  fractured  material  strength  surface.    For  tensile  mode,  𝜎𝑐 > 0,  these 
stress  components  are  reduced  to  zero.    For  compressive  mode,  𝜎𝑐 < 0,  the  normal 
stress  𝜎𝑐  is  assumed  to  deform  elastically  for  the  closed  matrix  crack.    Loading  on  the 
failure  envelop,  the  shear  stresses  are  assumed  to  ‘slide’  on  the  fractured  strength 
surface (frictional shear stresses) like in an ideal plastic material, while the subsequent 
unloading shear stress-strain path follows reduced shear moduli to the zero shear stress 
and strain state for both 𝜏𝑏𝑐 and 𝜏𝑐𝑎 components.
Material Models 
LS-DYNA Theory Manual 
(0)and 𝑆𝑏𝑐
The  post  failure  behavior  for  the  matrix  crack  in  the  a-c  plane  due  to  𝑓4  is 
modeled in the same fashion as that in the a-b plane as described  above.  In this case, 
(0)are reduced to zero instantaneously.  The post fracture 
when failure occurs, 𝑆𝑎𝑏
(0) = 0.  For tensile 
response is then governed by failure criterion of f5 with 𝑆𝑎𝑏
mode,  𝜎𝑏,  ,  𝜏𝑎𝑏  and  𝜏𝑏𝑐  are  zero.    For  compressive  mode,  𝜎𝑏 < 0,  𝜎𝑏  is  assumed  to  be 
elastic,  while  𝜏𝑎𝑏  and  𝜏𝑏𝑐  ‘slide’  on  the  fracture  strength  surface  as  in  an  ideal  plastic 
material, and the unloading path follows reduced shear moduli to the zero shear stress 
and  strain  state.    It  should  be  noted  that  𝜏𝑏𝑐  is  governed  by  both  the  failure  functions 
and should lie within or on each of these two strength surfaces. 
(0) = 0 and 𝑆𝑏𝑐
Fabric Lamina Model 
The  fiber  failure  criteria  of  Hashin  for  a  unidirectional  layer  are  generalized  to 
characterize  the  fiber  damage  in  terms  of  strain  components  for  a  plain  weave  layer.  
The  fill  and  warp  fiber  tensile/shear  failure  are  given  by  the  quadratic  interaction 
between the associated axial and shear stresses, i.e. 
𝑓6 = (
)
⟨𝜎𝑎⟩
𝑆𝑎T
+
(𝜏𝑎𝑏
2 + 𝜏𝑐𝑎
2 )
𝑆𝑎FS
− 1 = 0,
𝑓7 = (
⟨𝜎𝑏⟩
𝑆𝑏T
)
+
(𝜏𝑎𝑏
2 )
2 + 𝜏𝑏𝑐
𝑆𝑏FS
− 1 = 0,
(22.112.7)
(22.112.8)
where  𝑆𝑎T  and  𝑆𝑏T  are  the  axial  tensile  strengths  in  the  fill  and  warp  directions, 
respectively, and 𝑆𝑎FS and 𝑆𝑏FS are the layer shear strengths due to fiber shear failure in 
the fill and warp directions.  These failure criteria are applicable when the associated 𝜎𝑎 
or 𝜎𝑏 is positive.  It is assumed 𝑆aFS = SFS, and  
𝑆𝑏T
𝑆𝑎T
𝑆𝑏FS = SFS ∗
(22.112.9)
.
When 𝜎𝑎 or 𝜎𝑏is compressive, it is assumed that the in-plane compressive failure 
in both the fill and warp directions are given by the maximum stress criterion, i.e. 
𝑓8 = [
]
′⟩
⟨𝜎𝑎
𝑆𝑎C
𝑓9 = [
]
′⟩
⟨𝜎𝑏
𝑆𝑏C
− 1 = 0,
′ = −𝜎𝑎 + ⟨−𝜎𝑐⟩,
𝜎𝑎
(22.112.10)
− 1 = 0,
′ = −𝜎𝑏 + ⟨−𝜎𝑐⟩.
𝜎𝑏
(22.112.11)
where 𝑆𝑎C  and  𝑆𝑏C  are  the  axial  compressive  strengths  in  the  fill  and  warp  directions, 
respectively.  The crush failure under compressive pressure is 
𝑓10 = (
⟨𝑝⟩
𝑆FC
)
− 1 = 0,
𝑝 = −
𝜎𝑎 + 𝜎𝑏 + 𝜎𝑐
.
(22.112.12)
LS-DYNA Theory Manual 
Material Models 
A plain weave layer can fail under in-plane  shear stress without the occurrence 
of fiber breakage.  This in-plane matrix failure mode is given by 
𝑓11 = (
𝜏𝑎𝑏
𝑆𝑎𝑏
)
− 1 = 0,
(22.112.13)
where 𝑆𝑎𝑏 is the layer shear strength due to matrix shear failure. 
Another  failure  mode,  which  is  due  to  the  quadratic  interaction  between  the 
thickness stresses, is expected to be mainly a matrix failure.  This through the thickness 
matrix failure criterion is 
𝑓12 = 𝑆2 {(
)
⟨𝜎𝑐⟩
𝑆𝑐𝑇
+ (
𝜏𝑏𝑐
𝑆𝑏𝑐
)
+ (
𝜏𝑐𝑎
𝑆𝑐𝑎
)
} − 1 = 0,
(22.112.14)
where  𝑆𝑐T  is  the  through  the  thickness  tensile  strength,  and  𝑆𝑏𝑐,  and  𝑆𝑐𝑎  are  the  shear 
strengths assumed to depend on the compressive normal stress sc, i.e., 
{
𝑆𝑐𝑎
𝑆𝑏𝑐
}   =   {
(0)
𝑆𝑐𝑎
(0)} + tan(𝜑)⟨−𝜎𝑐⟩.
𝑆𝑏𝑐
(22.112.15)
When failure predicted by this criterion occurs within elements that are adjacent 
to  the  ply  interface,  the  failure  plane  is  expected  to  be  parallel  to  the  layering  planes, 
and,  thus,  can  be  referred  to  as  the  delamination  mode.    Note  that  a  scale  factor  𝑆  is 
introduced  to  provide  better  correlation  of  delamination  area  with  experiments.    The 
scale factor 𝑆 can be determined by fitting the analytical prediction to experimental data 
for the delamination area. 
Similar to the unidirectional model, when fiber tensile/shear failure is predicted 
in a layer by 𝑓6 or 𝑓7, the load carrying capacity of that layer in the associated direction is 
completely  eliminated.    For  compressive  fiber  failure  due  to  𝑓8  or  𝑓9,  the  layer  is 
assumed  to  carry  a  residual  axial  load  in  the  failed  direction,  while  the  load  carrying 
capacity  transverse  to  the  failed  direction  is  assumed  unchanged.    When  the 
compressive axial stress in a layer reaches the compressive axial strength 𝑆𝑎C or 𝑆𝑏C, the 
axial layer stress is assumed to be reduced to the residual strength 𝑆aRC or 𝑆bRC where 
𝑆aRC   =  SFFC ∗ SaC  and  SbRC   =  SFFC ∗ SbC.    The  axial  stress  is  assumed  to  remain 
constant, i.e., 𝜎𝑎 = −𝑆aCR or 𝜎𝑏 = −SbCR, for continuous compressive loading, while the 
subsequent  unloading  curve  follows  a  reduced  axial  modulus.    When  the  fiber  crush 
failure  has  occurred,  the  material  is  assumed  to  behave  elastically  for  compressive 
pressure, 𝑝 > 0, and to carry no load for tensile pressure, 𝑝 < 0. 
When the in-plane matrix shear failure is predicted by f11 the axial load carrying 
capacity within a failed element is assumed unchanged, while the in-plane shear stress 
is assumed to be reduced to zero.
Material Models 
LS-DYNA Theory Manual 
For  through  the  thickness  matrix  (delamination)  failure  given  by  equations  𝑓12, 
the  in-plane  load  carrying  capacity  within  the  element  is  assumed  to  be  elastic,  while 
(0), are set to zero.  For tensile mode, 
the strength values for the tensile mode, 𝑆𝑐𝑎
𝜎𝑐 > 0,  the  through  the  thickness  stress  components  are  reduced  to  zero.    For 
compressive  mode, 𝜎𝑐 < 0,  𝜎𝑐  is  assumed  to  be  elastic,  while  𝜏𝑏𝑐  and  𝜏𝑐𝑎  ‘slide’  on  the 
fracture strength surface as in an ideal plastic material, and the unloading path follows 
reduced shear moduli to the zero shear stress and strain state. 
(0)and 𝑆𝑏𝑐
The effect of strain-rate on the layer strength values of the fiber failure modes is 
modeled by the strain-rate dependent functions for the strength values {IRT} as 
{SRT } = {S0 } ( 1 + Crate1 ln
̇}
{ε̅
),
ε̇0
{𝑆RT } =
⎧𝑆𝑎T
⎫
}
{
}
{
𝑆𝑎C
}
{
}
{
𝑆𝑏T
⎬
⎨
𝑆𝑏C
}
{
}
{
𝑆FC
}
{
}
{
𝑆FS ⎭
⎩
 and  {𝜀̅
̇} =
⎧
{
{
{
{
{
⎨
{
{
{
{
{
⎩
∣𝜀̇𝑎∣
⎫
}
}
∣𝜀̇𝑎∣
}
}
∣𝜀̇𝑏∣
}
∣𝜀̇𝑏∣
⎬
}
∣𝜀̇𝑐∣
}
}
}
}
2 )
2 + 𝜀̇𝑏𝑐
2⎭
(𝜀̇𝑐𝑎
, 
(22.112.16)
(22.112.17)
where 𝐶rate is the strain-rate constants, and {𝑆0 }are the strength values of {𝑆RT } at the 
reference strain-rate 𝜀̇0. 
Damage Model 
The damage model is a generalization of the layer failure model of Material 161 
by  adopting  the  MLT  damage  mechanics  approach,  Matzenmiller  et  al.    [1995],  for 
characterizing  the  softening  behavior  after  damage  initiation.    Complete  model 
description is given in Yen [2001].  The damage functions, which are expressed in terms 
of  ply  level  engineering  strains,  are  converted  from  the  above  failure  criteria  of  fiber 
and matrix failure modes by neglecting the Poisson’s effect.  Elastic moduli reduction is 
expressed in terms of the associated damage parameters 𝜛𝑖: 
′ = (1 − ϖ𝑖)E𝑖
E𝑖
(22.112.18)
𝑚𝑖/𝑚𝑖)  𝑟𝑖 ≥ 0  𝑖 = 1, . . . ,6, 
ϖ𝑖 = 1 − exp(−𝑟𝑖
(22.112.19)
′  are  the  reduced  elastic  moduli,  𝑟𝑖  are  the 
where  𝐸𝑖  are  the  initial  elastic  moduli,  𝐸𝑖
damage  thresholds  computed  from  the  associated  damage  functions  for  fiber  damage, 
matrix  damage  and  delamination,  and  mi  are  material  damage  parameters,  which  are 
currently assumed to be independent of strain-rate.  The damage function is formulated 
to  account  for  the  overall  nonlinear  elastic  response  of  a  lamina  including  the  initial 
‘hardening’ and the subsequent softening beyond the ultimate strengths. 
In  the  damage  model  (Material  162),  the  effect  of  strain-rate  on  the  nonlinear 
stress-strain  response  of  a  composite  layer  is  modeled  by  the  strain-rate  dependent 
functions for the elastic moduli {𝐸RT } as
LS-DYNA Theory Manual 
Material Models 
{𝐸RT } = {𝐸0 } ( 1 + {𝐶rate} ln
̇}
{𝜀̅
),
𝜀̇0
{𝐸RT } =
⎧ 𝐸𝑎
⎫
}}
{{
𝐸𝑏
}}
{{
𝐸𝑐
⎬
⎨
𝐺𝑎𝑏
}}
{{
𝐺𝑏𝑐
}}
{{
𝐺𝑐𝑎⎭
⎩
 , {𝜀̅
̇} =
⎧ ∣𝜀̇𝑎∣
⎫
}
{
}
{
∣𝜀̇𝑏∣
}
{
}
{
∣𝜀̇𝑐∣
⎬
⎨
∣𝜀̇𝑎𝑏∣
}
{
}
{
∣𝜀̇𝑏𝑐∣
}
{
}
{
∣𝜀̇𝑐𝑎∣⎭
⎩
 and {𝐶rate} =
⎧𝐶rate2
⎫
}
{
}
{
𝐶rate2
}
{
}
{
𝐶rate4
⎬
⎨
𝐶rate3
}
{
}
{
𝐶rate3
}
{
}
{
𝐶rate3⎭
⎩
, 
(22.112.20)
(22.112.21)
where {𝐶rate} are the strain-rate constants.  {𝐸0} are the modulus values of {𝐸RT } at the 
reference strain-rate 𝜀̇0.
Material Models 
LS-DYNA Theory Manual 
22.113  Material Model 163:  Modified Crushable Foam 
The  volumetric  strain  is  defined  in  terms  of  the  relative  volume,  𝑉,  as:  𝛾 =
 1. −𝑉.  The relative volume is defined as the ratio of the current to the initial volume.  
In place of the effective plastic strain in the D3PLOT database, the integrated volumetric 
strain is output. 
This  material  is  an  extension  of  material  63,  *MAT_CRUSHABLE_FOAM.    It 
allows  the  yield  stress  to  be  a  function  of  both  volumetric  strain  rate  and  volumetric 
strain. 
  Rate  effects  are  accounted  for  by  defining  a  table  of  curves  using 
*DEFINE_TABLE.    Each  curve  defines  the  yield  stress  versus  volumetric  strain  for  a 
different  strain  rate.    The  yield  stress  is  obtained  by  interpolating  between  the  two 
curves that bound the strain rate. 
To  prevent  high  frequency  oscillations  in  the  strain  rate  from  causing  similar 
high frequency oscillations in the yield stress, a modified volumetric strain rate is used 
when  interpolating  to  obtain  the  yield  stress.    The  modified  strain  rate  is  obtained  as 
follows.  If NCYCLE is > 1, then the modified strain rate is obtained by a time average 
of the actual strain rate over NCYCLE solution cycles.  For SRCLMT > 0, the modified 
strain rate is capped so that during each cycle, the modified strain rate is not permitted 
to change more than SRCLMT multiplied by the solution time step.
Figure  22.113.1.    Rate  effects  are  defined  by  a  family  of  curves  giving  yield
stress versus volumetric strain. 
1-V
LS-DYNA Theory Manual 
Material Models 
22.114  Material Model 164:  Brain Linear Viscoelastic 
The shear relaxation behavior is described by the Maxwell model as: 
𝐺(𝑡) = 𝐺 + (𝐺0 − 𝐺∞)𝑒−𝛽𝑡.
(22.114.1)
A Jaumann rate formulation is used 
𝛻
𝜎′𝑖𝑗
= 2 ∫ 𝐺(𝑡 − 𝜏) 𝐷′𝑖𝑗(𝜏)𝑑𝑡
.
(22.114.2)
𝛻
where the prime denotes the deviatoric part of the stress rate, 𝜎
.  For the Kelvin model the stress evolution equation is defined as: 
𝑖𝑗, and the strain rate 𝐷𝑖𝑗 
𝑠 ̇𝑖𝑗 +
𝑠𝑖𝑗 = (1 + 𝛿𝑖𝑗) (𝐺0 +
𝐺∞
) 𝑒 ̇𝑖𝑗.
(22.114.3)
The strain data as written to the LS-DYNA database may be used to predict damage, see 
[Bandak 1991].
Material Models 
LS-DYNA Theory Manual 
22.115  Material Model 166:  Moment Curvature Beam 
Curvature rate can be decomposed into elastic part and plastic part: 
𝜀̇ = 𝜀̇e + 𝜀̇p   ⇒  
𝜀̇
=
𝜀̇p
+
𝜀̇p
⇒ 𝜅̇ = 𝜅̇e + 𝜅p.
(22.115.1)
Moment rate is the product of elastic bending stiffness and elastic curvature: 
𝑀̇ = ∫ 𝜎̇ 𝑦𝑑𝐴
= ∫ 𝐸e𝜀̇e𝑦𝑑𝐴
= ∫ 𝐸e𝜅̇e𝑦2𝑑𝐴
= ∫ 𝐸e(𝜅̇ − 𝜅̇p)𝑦2𝑑𝐴
= 𝐸e(𝜅̇ − 𝜅̇p) ∫ 𝑦2𝑑𝐴 = (𝐸𝐼)e(𝜅̇ − 𝜅̇p)
.
Plastic flow rule: 𝜓 = |𝑀| (Isotropic hardening) 
(22.115.2)
𝜅̇p = 𝜆̇
𝜕𝜓
𝜕𝑀
Yield condition: 
= 𝜆̇sign(𝑀), 𝜅̅
̇p = √𝜅̇p𝜅̇p = 𝜆̇.
(22.115.3)
𝑓 = |𝑀| − 𝑀Y(𝜅̅p) = 0.
Loading and unloading conditions: 
𝜆̇ ≥ 0, 𝑓 ≤ 0, 𝜆̇𝑓 = 0.
Consistency condition: 
𝑓 ̇ = 0 ⇒ 𝑀̇  sign(𝑀) −
̇p 
⇒   𝜆̇ ≡ 𝜅̅
𝑀sign(𝑀)
(𝐸𝐼)p =
=
∂𝑀Y
∂𝜅̅p 𝜅̅p = 0
(𝐸𝐼)e
(𝐸𝐼)p (𝜅̇ − 𝜅̇p) sign(𝑀) 
=
(𝐸𝐼)e
(𝐸𝐼)p [𝜅̇ − 𝜆̇ sign(𝑀)]sign(𝑀) 
̇ =
(𝐸𝐼)e𝜅̇ sign(𝑀)
(𝐸𝐼)p + (𝐸𝐼)e
 ⇒   𝜆̇ ≡ 𝜅̅
(22.115.4)
(22.115.5)
(22.115.6)
Moment  rate  is  also  the  product  of  tangential  bending  stiffness  and  total 
curvature: 
𝑀̇ = (𝐸𝐼)ep𝜅̇.
(22.115.7)
Elastic, plastic, and tangential stiffnesses are obtained from user-defined curves: 
(𝐸𝐼)ep =
𝑑𝑀
𝑑𝜅
,
(𝐸𝐼)p =
𝑑𝑀
𝑑𝜅̅p.
(22.115.8)
Both are obtained from user-defined curves.
LS-DYNA Theory Manual 
Material Models 
(𝐸𝐼)ep(𝐸𝐼)p
(𝐸𝐼)p − (𝐸𝐼)ep.
For  Torsion-Twist,  simply  replace  𝑀  by  𝑇,  𝜅  by  𝛽,  (𝐸𝐼)  by  (𝐺𝐽).    For  Force-Strain, 
simply replace 𝑀 by 𝑁, 𝜅 by 𝜀, (𝐸𝐼) by (𝐸𝐴).
(𝐸𝐼)e =
(22.115.9)
Material Models 
LS-DYNA Theory Manual 
22.116  Material Model 169:  Arup Adhesive 
The through-thickness direction is identified from the smallest dimension of each 
element.    It  is  expected  that  this  dimension  will  be  much  smaller  than  in-plane 
dimensions (typically 2mm compared with 10mm). 
In-plane  stresses  are  set  to  zero:  it  is  assumed  that  the  stiffness  and  strength  of 
the substrate is large compared with that of the adhesive, given the relative thicknesses.  
If  the  substrate  is  modeled  with  shell  elements,  it  is  expected  that  these  will  lie  at  the 
mid-surface  of  the  substrate  geometry.    Therefore  the  solid  elements  representing  the 
adhesive will be thicker than the actual bond.  The yield and failure surfaces are treated 
as  a  power-law  combination  of  direct  tension  and  shear  across  the  bond:  (𝜎/
𝜎max)PWRT + (𝜏/𝜏max)PWRS = 1.0  at  yield.    The  stress-displacement  curves  for  tension 
and  shear  are  shown  in  the  diagrams  below.    In  both  cases,  𝐺c  is  the  area  under  the 
curve.    Because  of  the  algorithm  used,  yielding  in  tension  across  the  bond  does  not 
require strains in the plane of the bond – unlike the plasticity models, plastic flow is not 
treated as volume-conserving.  
The Plastic Strain output variable has a special meaning: 
•  0 < ps < 1: ps is the maximum value of the yield function experienced since time 
zero 
•   
1 < ps < 2:  the  element  has  yielded  and  the  strength  is  reducing  towards 
failure – yields at ps = 1, fails at ps = 2.
Stress
Stress
TENMAX
SHRMAX
Area = Gcten
Failure
dp = SHRP.dfs
Area = Gcshr
Failure
dft
Displacement
Tension
dp
Shear
dfs
Displacement
Figure 22.116.1.
LS-DYNA Theory Manual 
Material Models 
22.117  Material Model 170: Resultant Anisotropic 
The in-plane elastic matrix for in-plane plane stress behavior is given by: 
𝐂in plane =
𝑄11p 𝑄12p
⎡
𝑄12p 𝑄22p
⎢
⎢
⎢
⎢
⎢
⎣
𝑄44p
𝑄55p 
⎤
⎥
⎥
. 
⎥
⎥
⎥
𝑄66p⎦
The terms Q𝑖𝑗p are defined as: 
𝑄11p =
𝑄22p =
𝑄12p =
𝐸11p
1 − 𝜈12p𝜈21p
𝐸22p
1 − 𝜈12p𝜈21p
𝜈12p𝐸11p
1 − 𝜈12p𝜈21p
,
, 
, 
𝑄44p = 𝐺12p, 
𝑄55p = 𝐺23p, 
𝑄66p = 𝐺31p.
The elastic matrix for bending behavior is given by: 
𝐂bending =
𝑄11b 𝑄12b
𝑄12b  𝑄22b
⎡
⎢
⎣
⎤. 
⎥
𝑄44b⎦
The terms 𝑄𝑖𝑗b are similarly defined.
(22.117.1)
(22.117.2)
(22.117.3)
Material Models 
LS-DYNA Theory Manual 
22.118  Material Model 175:  Viscoelastic Maxwell 
Rate  effects  are  taken  into  accounted  through  linear  viscoelasticity  by  a 
convolution integral of the form: 
𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏)
𝜕𝜀𝑘𝑙
𝜕𝜏
𝑑𝜏
,
(22.118.1)
where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) is the relaxation function for different stress measures.  This stress is 
added to the stress tensor determined from the strain energy functional.   
If  we  wish  to  include  only  simple  rate  effects,  the  relaxation  function  is 
represented by six terms from the Prony series: 
𝑔(𝑡) = ∑ 𝐺𝑚𝑒−𝛽𝑚𝑡
𝑚=1
.
(22.118.2)
We characterize this in the input by shear moduli, 𝐺𝑖, and the decay constants, 𝛽𝑖.  
An  arbitrary  number  of  terms,  up  to  6,  may  be  used  when  applying  the  viscoelastic 
model. 
For  volumetric  relaxation,  the  relaxation  function  is  also  represented  by  the 
Prony series in terms of bulk moduli: 
𝑘(𝑡) = ∑ 𝐾𝑚𝑒−𝛽𝑘𝑚𝑡
.
𝑚=1
(22.118.3)
The Arrhenius and Williams-Landau-Ferry (WLF) shift functions account for the 
effects of the temperature on the stress relaxation.  A scaled time, 𝑡′, 
𝑡′ = ∫ 𝛷(𝑇)𝑑𝑡
,
(22.118.4)
is  used  in  the  relaxation  function  instead  of  the  physical  time.    The  Arrhenius  shift 
function is 
𝛷(𝑇) = exp (−𝐴 {
−
𝑇REF
}),
and the Williams-Landau-Ferry shift function is 
𝛷(𝑇) = exp (−𝐴
𝑇 − TREF
𝐵 + 𝑇 − 𝑇REF
).
(22.118.5)
(22.118.6)
LS-DYNA Theory Manual 
Material Models 
22.119  Material Model 176:  Quasilinear Viscoelastic 
The equations for this model are given as: 
𝜎(𝑡) = ∫ 𝐺(𝑡 − 𝜏)
𝜕𝜎𝜀[𝜀(𝜏)]
𝜕𝜀
𝜕𝜀
𝜕𝜏
𝑑𝜏, 
𝐺(𝑡) = ∑ 𝐺𝑖
𝑖=1
𝜎𝜀(𝜀) = ∑ 𝐶𝑖
𝑖=1
𝑒−𝛽𝑡, 
𝜀𝑖,
(22.119.1)
where  G  is  the  shear  modulus.    In  place  of  the  effective  plastic  strain  in  the  D3PLOT 
database, the effective strain is output:  
𝜀effective = √
𝜀𝑖𝑗𝜀𝑖𝑗.
(22.119.2)
The  polynomial  for  instantaneous  elastic  response  should  contain  only  odd  terms  if 
symmetric tension-compression response is desired.
Material Models 
LS-DYNA Theory Manual 
22.120  Material Models 177 and 178:  Hill Foam and 
Viscoelastic Hill Foam 
22.120.1  Hyperelasticity Using the Principal Stretch Ratios 
Material types 177 and 178 in LS-DYNA are highly compressible Ogden models 
combined  with  viscous  stress  contributions.    The  latter  model  also  allows  for  an 
additive  viscoelastic  stress  contribution.    As  for  the  rate  independent  part,  the 
constitutive law is determined by a strain energy function that is expressed in terms of 
the principal stretches, i.e., 𝑊 = 𝑊(𝜆1, 𝜆2, 𝜆3). To obtain the Cauchy stress 𝜎𝑖𝑗, as well as 
TC,  they  are  first  calculated  in  the  principal  basis 
the  constitutive  tensor  of  interest,  𝐶𝑖𝑗𝑘𝑙
after  which  they  are  transformed  back  to  the  “base  frame”,  or  standard  basis.    The 
complete set of formulas is given by Crisfield [1997] and is for the sake of completeness 
recapitulated here. 
The principal Kirchhoff stress components are given by 
E = 𝜆𝑖
𝜏𝑖𝑖
𝜕𝑊
𝜕𝜆𝑖
(no sum),
that are transformed to the standard basis using the standard formula 
E.
𝜏𝑖𝑗 = 𝑞𝑖𝑘𝑞𝑗𝑙𝜏𝑘𝑙
(22.120.1)
(22.120.2)
The 𝑞𝑖𝑗 are the components of the orthogonal tensor containing the eigenvectors 
of the principal basis.  The Cauchy stress is then given by  
𝜎𝑖𝑗 = 𝐽−1𝜏𝑖𝑗,
(22.120.3)
where 𝐽 = 𝜆1𝜆2𝜆3 is the relative volume change. 
The  constitutive  tensor  that  relates  the  rate  of  deformation  to  the  Truesdell 
(convected) rate of Kirchhoff stress in the principal basis can be expressed as 
TKE = 𝜆𝑗
𝐶𝑖𝑖𝑗𝑗
TKE =
𝐶𝑖𝑗𝑖𝑗
TKE =
𝐶𝑖𝑗𝑖𝑗
E𝛿𝑖𝑗
− 2𝜏𝑖𝑖
𝜕𝜏𝑖𝑖
𝜕𝜆𝑗
2𝜏𝑗𝑗
E − 𝜆𝑖
2𝜏𝑖𝑖
𝜆𝑗
2 − 𝜆𝑗
𝜆𝑖
𝜕𝜏𝑖𝑖
(
𝜕𝜆𝑖
𝜆𝑖
−
𝜕𝜏𝑖𝑖
𝜕𝜆𝑗
,    𝑖 ≠ 𝑗, 𝜆𝑖 ≠ 𝜆𝑗
),
𝑖 ≠ 𝑗, 𝜆𝑖 = 𝜆𝑗
⎫
}
}
}
}
}
}
⎬
}
}
}
}
}
}
⎭
   (no sum). 
(22.120.4)
These components are transformed to the standard basis according to
LS-DYNA Theory Manual 
Material Models 
TK = 𝑞𝑖𝑝𝑞𝑗𝑞𝑞𝑘𝑟𝑞𝑙𝑠𝐶𝑝𝑞𝑟𝑠
TKE,
𝐶𝑖𝑗𝑘𝑙
(22.120.5)
and finally the constitutive tensor relating the rate of deformation to the Truesdell rate 
of Cauchy stress is obtained through 
TC = 𝐽−1𝐶𝑖𝑗𝑘𝑙
TK.
𝐶𝑖𝑗𝑘𝑙
(22.120.6)
22.120.2  Hill’s Strain Energy Function 
The strain energy function for materials 177 and 178 is given by 
𝑊 = ∑
𝑚=1
𝜇𝑚
𝛼𝑚
[𝜆1
𝛼𝑚 + 𝜆2
𝛼𝑚 + 𝜆3
𝛼𝑚 − 3 +
(𝐽−𝑛𝛼𝑚 − 1)]
.
(22.120.7)
where  𝑛,  𝜇𝑚  and  𝛼𝑚  are  material  parameters.    To  apply  the  formulas  in  the  previous 
section, we require 
E = 𝜆𝑖
𝜏𝑖𝑖
𝜕𝑊
𝜕𝜆𝑖
= ∑
𝑚=1
𝜇𝑚
𝛼𝑚 − 𝐽−𝑛𝛼𝑚).
(𝜆𝑖
Proceeding with the constitutive tensor, we have 
𝜆𝑗
𝜕𝜏𝑖𝑖
𝜕𝜆𝑗
= ∑ 𝜇𝑚𝛼𝑚(𝜆𝑖
𝛼𝑚𝛿𝑖𝑗 + 𝑛𝐽−𝑛𝛼𝑚)
.
𝑚=1
(22.120.8)
(22.120.9)
In addition to the hyperelastic stress described above, a viscous stress is added.  
Converting to Voigt notation, this stress can be written, 
𝛔 = 𝐂𝐃,
(22.120.10)
where  𝛔  denotes  Cauchy  stress,  𝐃  is  the  rate-of-deformation  and  𝐂  is  an  isotropic 
constitutive  matrix  representing  the  viscosity.    In  element  m,  the  constitutive  matrix 
depends on the element deformation according to 
𝐂 =
𝑑𝑚
𝐂𝟎,
(22.120.11)
where  𝑑𝑚  is  the  diameter4  of  element  m  and  𝐂𝟎  is  a  constitutive  matrix  that  depends 
only  on  the  material  parameters.    The  stress  contribution  to  the  internal  force  can  be 
written 
𝑓 int = ∫ 𝐁T𝛔𝑑𝛺𝑚,
𝛺𝑚
(22.120.12)
and the corresponding material time derivative is 
4 Experiments indicate that d(cid:2923) is the smallest dimension of the element.
Material Models 
LS-DYNA Theory Manual 
𝑓 ̇mat = ∫ 𝐁T𝛔∇𝑇𝑑𝛺𝑚
.
𝛺𝑚
(22.120.13)
Here 𝛺𝑚 is the current configuration of element m, 𝐁 is the strain-displacement matrix 
and ∇𝑇 denotes the Truesdell rate of Cauchy stress.  The aim is to identify the material 
tangent modulus through 
𝑓 ̇mat = ∫ 𝐁T𝐂mat𝐁𝑑𝛺𝑚
𝑢̇,
𝛺𝑚
(22.120.14)
for the viscous stress with u̇ being the nodal velocity.  The Truesdell rate of the viscous 
stress can be written, 
𝛔𝛁𝐓 = 𝐂̇𝐃 + 𝐂𝐃̇ + tr(𝐃)𝛔 − 𝐋𝛔 − 𝛔𝐋𝐓,
(22.120.15)
where  Lis  the  velocity  gradient.    The  terms  on  the  right  hand  side  can  be  treated  as 
follows. 
For the first term, we can assume that 𝑑𝑚 ∝ J1/3 and then approximate  
𝐂̇ = −
tr(𝐃)𝐂.
(22.120.16)
Using Equation (22.120.10), Equation (22.120.13), the first term on the right hand 
side of Equation (22.120.15), Equation (22.120.16) and the expression  
𝐃 = 𝐁𝐮̇,
(22.120.17)
a material tangent modulus contribution can be identified in Equation (22.120.14) as 
−
𝛔𝛅T,
(22.120.18)
where 𝛅 denotes the identity matrix in Voigt notation.  
For the second term in Equation (22.120.15), we differentiate Equation (22.120.17) 
to see that 
𝐃̇ = 𝐁̇𝐮̇ + 𝐁𝐮̈.
(22.120.19)
Post-poning the treatment of the first term, the second of these two terms can be 
treated easily as this gives the following contribution to the material time derivative  
∫ 𝐁T𝐂𝐁𝑑𝛺𝑚𝑢̇
𝛺𝑚
𝛽Δ𝑡
,
(22.120.20)
where γ and 𝛽 are parameters in the Newmark scheme and Δ𝑡 is the time step.  From 
this  expression,  a  material  tangent  modulus  can  through  Equation  (22.120.14)  be 
identified as,
LS-DYNA Theory Manual 
Material Models 
𝐂mat =
𝛽Δ𝑡
𝐂.
(22.120.21)
The  third  term  in  Equation  (22.120.15)  contributes  to  the  material  tangent 
modulus as 
resulting in a material tangent modulus given so far by 
𝛔𝛅T
𝛽Δ𝑡
𝐂 +
𝛔𝛅T.
22.120.3  Viscous Stress 
(22.120.22)
(22.120.23)
From the remaining terms, i.e., the last two terms in Equation (22.120.15) and the 
first  term  in  Equation  (22.120.19),  we  see  it  impossible  to  identify  contributions  to  a 
material tangent modulus.  We believe that these terms must be treated in some other 
manner.  We are thus left with two choices, either to approximate these terms within the 
existing  framework  or  to  attempt  a  thorough  implementation  of  the  correct  tangent 
stiffness using a different, and probably demanding, approach.  We reason as follows.  
Since  this  stress  contribution  is  viscous  and  proportional  to  the  mesh  size,  it  is 
our belief that it serves as a stabilizing stress in the occurrence of a coarse mesh and/or 
large  deformation  rates,  and  really  has  little  or  nothing  to  do  with  the  actual  material 
models.  If only the simulation process is slow (which it often is in an implicit analysis) 
and/or  the  mesh  is  sufficiently  fine,  this  stress  should  be  negligible  compared  to  the 
other  stress(es).    With  this  in  mind,  we  feel  that  it  is  not  crucial  to  derive  an  exact 
tangent  for  this  stress  but  we  can  be  satisfied  with  an  approximation.    Even  if 
attempting  a  more  thorough  derivation  of  the  tangent  stiffness,  we  would  most 
certainly have to make approximations along the way.  Hence we do not see this as an 
attractive approach.  
In  the  implementation  we  have  simply  neglected  all  terms  involving  stresses 
since  the  experience  from  earlier  work  is  that  such  terms  generally  have  a  negative 
effect  on  the  tangent  if  they  are  not  absolutely  correct.    In  addition,  most  of  the  terms 
involving  stresses  contribute  to  a  nonsymmetric  tangent  stiffness,  which  cannot  be 
supported  by  LS-DYNA  at  the  moment.    Hence  the  material  tangent  modulus  for  the 
viscous stress is given by Equation (22.120.21). We are aware of that this may be a crude 
approximation, and if experiments show that it is a poor one, we will take a closer look 
at it. 
In material type 178, the viscous stress acts only in the direction of the principal 
stretches and in compression.  With C being an isotropic tensor, we evaluate the tangent 
stiffness modulus in the principal basis according to Equation (22.120.21), modify it to
Material Models 
LS-DYNA Theory Manual 
account for the mentioned conditions and then transform it back to the global frame of 
reference. 
22.120.4  Viscoelastic Stress Contribution 
For material 178, an optional viscoelastic stress contribution can be added.  The 
evolution of this stress in time can be stated as 
where 
12
∇ = ∑ 2𝐺𝑚𝑠𝑖𝑗
𝜎𝑖𝑗
𝑚=1
m∇
,
m,
m∇ = 𝐷𝑖𝑗 − 𝛽𝑚𝑠𝑖𝑗
𝑠𝑖𝑗
(22.120.24)
(22.120.25)
Here  𝐺𝑚  and  𝛽𝑚  are  material  constants,  and  𝐷𝑖𝑗  is  the  rate-of-deformation  tensor.  
Referring  to  Borrvall  [2002],  we  state  that  the  tangent  stiffness  modulus  for  this  stress 
contribution can be written 
12
𝐶𝑖𝑗𝑘𝑙 = ∑ 𝐺𝑚
(𝛿𝑖𝑘𝛿𝑗𝑙 + 𝛿𝑖𝑙𝛿𝑗𝑘).
𝑚=1
(22.120.26)
Just  as  for  the  viscous  stress,  this  stress  acts  only  in  the  direction  of  the  principal 
stretches.    Hence  the  tangent  modulus  is  formed  in  the  principal  basis,  modified  to 
account for this condition and then transformed back to the global frame of reference. 
22.120.5  Material Tangent Modulus for the Fully Integrated Brick 
To avoid locking tendencies for the fully integrated brick element in LS-DYNA, 
the stress is modified as 
𝛔S/R = 𝛔 + (𝑝 − 𝑝̅)𝐈,
(22.120.27)
where  𝑝  is  the  pressure  and  𝑝̅  is  the  mean  pressure  in  the  element.    This  affects  the 
tangent  stiffness  since  one  has  to  take  into  account  that  the  pressure  is  constant  in the 
element.  Deriving the material time derivative of the internal force results in 
𝑓 ̇mat = ∫ 𝐁T𝐂𝐁𝑑𝛺𝑚
𝑢̇ + ∫ (𝑝 − 𝑝̅)𝐁T(𝐈 ⊗ 𝐈)𝐁𝑑𝛺𝑚
𝑢̇
𝛺𝑚
𝛺𝑚
                 −2 ∫ (𝑝 − 𝑝̅)𝐁T𝐁𝑑𝛺𝑚
𝛺𝑚
𝑢̇ + ∫ (ṗ − p̅̅̅̅̇)BTdΩm
. 
Ωm
(22.120.28)
To  implement  this  tangent,  the  last  term  is  the  most  difficult  to  deal  with  as  it 
involves the time derivative (or variation) of the pressure.  For certain types of material 
models,  for  instance  material  type  77  in  LS-DYNA,  the  pressure  is  a  function  of  the 
relative volume 
22-282 (Material Models) 
𝑝 = 𝑝(𝐽),
LS-DYNA Theory Manual 
Material Models 
and with the approximation 
𝑝̅ = 𝑝(𝐽 ̅),
the last term can be evaluated to 
∫ 𝐽𝑝′(𝐽)𝐁T(𝐈 ⊗ 𝐈)𝐁𝑑𝛺𝑚𝑢̇
𝛺𝑚
− ∫ 𝐽 ̅𝑝′(𝐽 ̅)𝐁̅̅̅̅̅T(𝐈 ⊗ 𝐈)𝐁̅̅̅̅̅𝑑𝛺𝑚𝑢̇
,
𝛺𝑚
(22.120.30)
(22.120.31)
and a symmetric tangent stiffness can quite easily be implemented.  We have here used 
𝐽 ̅ and 𝐁̅̅̅̅̅ for the mean values of 𝐽 and 𝐁, respectively.  For other types of material models, 
such  as  the  ones  described  in  this  document  or  material  type  27  in  LS-DYNA,  the 
expression for the pressure is more complicated.  A characterizing feature is that a non-
zero  pressure  can  occur  under  constant  volume.    This  will  in  general  complicate  the 
implementation  of  the  last  term  and  will  also  contribute  to  a  non-symmetric  tangent 
stiffness  that  cannot  be  handled  in  LS-DYNA  at  the  moment.    For  material  27, 
neglecting  this  had  a  tremendous  impact  on  the  performance  of  the  implicit  solution 
procedure, .  For the current material models, it seems to be of less 
importance, and we believe that this is due to the higher compressibility allowed. 
22.120.6  Viscous damping 
Viscous  damping in the model follows an implementation identical to that of material 
type 57.
Material Models 
LS-DYNA Theory Manual 
22.121  Material Models 179 and 180:  Low Density Synthetic 
Foam 
Material types 179 and 180 in LS-DYNA are highly compressible synthetic foam 
models  with  no  Poisson’s  ratio  effects  combined  with  an  optional  visco-elastic  and  a 
stabilizing  viscous  stress  contribution.    The  tensile  behavior  of  the  materials  is  linear 
where  the  stress  cannot  exceed  a  user  prescribed  cutoff  stress.    In  compression  the 
materials  show  a  hysteresis  on  unloading  similar  to  material  57.  In  addition,  the  first 
load  cycle  damages  the  material  so  that  the  stress  level  on  reloading  is  significantly 
reduced.    For  material  179  the  damage  is  isotropic  while  it  is  orthotropic  for  material 
180.  Viscous  damping  in  the  model  follows  an  implementation  identical  to  that  of 
material type 57. 
22.121.1  Hyperelasticity Using the Principal Stretch Ratios 
As  for  the  rate  independent  part  of  the  stress,  the  constitutive  law  is  mainly 
determined  by  a  strain  energy  function  that  is  expressed  in  terms  of  the  principal 
stretches,  i.e.,  𝑊 = 𝑊(𝜆1, 𝜆2, 𝜆3).  To  obtain  the  Cauchy  stress  𝜎𝑖𝑗,  as  well  as  the 
TC,  they  are  first  calculated  in  the  principal  basis  after 
constitutive  tensor of  interest, 𝐶𝑖𝑗𝑘𝑙
which they are transformed back to the “base frame”, or standard basis.  The complete 
set  of  formulas  is  given  by  Crisfield  [1997]  and  is  for  the  sake  of  completeness 
recapitulated here. 
The principal Kirchhoff stress components are given by 
E = 𝜆𝑖
𝜏𝑖𝑖
𝜕𝑊
𝜕𝜆𝑖
(no sum),
that are transformed to the standard basis using the standard formula 
E.
𝜏𝑖𝑗 = 𝑞𝑖𝑘𝑞𝑗𝑙𝜏𝑘𝑙
(22.121.1)
(22.121.2)
The 𝑞𝑖𝑗 are the components of the orthogonal tensor containing the eigenvectors 
of the principal basis.  The Cauchy stress is then given by , 
𝜎𝑖𝑗 = 𝐽−1𝜏𝑖𝑗,
(22.121.3)
where 𝐽 = 𝜆1𝜆2𝜆3 is the relative volume change. 
The  constitutive  tensor  that  relates  the  rate  of  deformation  to  the  Truesdell 
(convected) rate of Kirchhoff stress can in the principal basis be expressed as
LS-DYNA Theory Manual 
Material Models 
TKE = 𝜆𝑗
𝐶𝑖𝑖𝑗𝑗
TKE =
𝐶𝑖𝑗𝑖𝑗
TKE =
𝐶𝑖𝑗𝑖𝑗
E𝛿𝑖𝑗
− 2𝜏𝑖𝑖
𝜕τii
𝜕𝜆𝑗
2𝜏𝑗𝑗
E − 𝜆𝑖
2𝜏𝑖𝑖
𝜆𝑗
2 − 𝜆𝑗
𝜆𝑖
𝜕𝜏𝑖𝑖
(
𝜕𝜆𝑖
𝜆𝑖
−
𝜕𝜏𝑖𝑖
𝜕𝜆𝑗
),
𝑖 ≠ 𝑗, 𝜆𝑖 = 𝜆𝑗
,    𝑖 ≠ 𝑗, 𝜆𝑖 ≠ 𝜆𝑗
 (no sum). 
(22.121.4)
These components are transformed to the standard basis according to 
TK = 𝑞𝑖𝑝𝑞𝑗𝑞𝑞𝑘𝑟𝑞𝑙𝑠𝐶𝑝𝑞𝑟𝑠
TKE,
𝐶𝑖𝑗𝑘𝑙
(22.121.5)
and finally the constitutive tensor relating the rate of deformation to the Truesdell rate 
of Cauchy stress is obtained through. 
TC = 𝐽−1𝐶𝑖𝑗𝑘𝑙
TK .
𝐶𝑖𝑗𝑘𝑙
(22.121.6)
22.121.2  Strain Energy Function 
The strain energy function for materials 179 and 180 is given by  
,
W = ∑ 𝑤(λm)
m=1
(22.121.7)
where 
𝑤(𝜆) =
2𝐸
(𝜆 − 1)2
⎧𝑠 (𝜆 − 1 −
{{{{{
{{{{{
∫ 𝑓s(1 − 𝜇)𝑑𝜇
⎨
⎩
) if  𝜆 ≥
+ 1
if  1 ≤ 𝜆 <
otherwise
+ 1
(22.121.8)
Here  s  is  the  nominal  tensile  cutoff  stress  and  𝐸  is  the  stiffness  coefficient  relating  a 
change in principal stretch to a corresponding change in nominal stress.  The function 
𝑓s(≤ 0) gives the nominal compressive stress as a function of the strain in compression 
for the second and all subsequent load cycles and is supplied by the user.  To apply the 
formulas in the previous section, we require 
E = 𝜆𝑖
𝜏𝑖𝑖
𝜕𝑤
𝜕𝜆𝑖
=
if  𝜆𝑖 ≥
+ 1
𝐸𝜆𝑖(𝜆𝑖 − 1)
if  1 ≤ 𝜆𝑖 <
𝜆𝑖𝑓𝑠(1 − 𝜆𝑖) otherwise
⎧𝑠𝜆𝑖
{{{
⎨
{{{
⎩
+ 1
(22.121.9)
Proceeding with the constitutive tensor, we have
Material Models 
LS-DYNA Theory Manual 
𝜆𝑗
𝜕𝜏𝑖𝑖
𝜕𝜆𝑗
= 𝛿𝑖𝑗
⎧𝑠𝜆𝑖
{{{
⎨
{{{
⎩
𝐸𝜆𝑖(2𝜆𝑖 − 1)
if  1 ≤ 𝜆𝑖 <
𝜆𝑖(𝑓𝑠(1 − 𝜆𝑖) − 𝜆𝑖𝑓 ′𝑠(1 − 𝜆𝑖)) otherwise
if 𝜆𝑖 ≥
+ 1
+ 1
(22.121.10)
22.121.3  Modeling of the Hysteresis 
The hyperelastic part of the Cauchy stress is scaled by a factor 𝜅 given by 
where 
𝜅 =
,
𝐸̅̅̅̅
𝐸 = ∫ 𝐽𝛔: 𝑑𝛆,
is the stored energy in the material and 
𝐸̅̅̅̅ = 𝐸maxexp(−𝛽(𝑡 − 𝑠)).
(22.121.11)
(22.121.12)
(22.121.13)
Here 𝑠 stands for the time point when E has its maximum 𝐸max in the interval [0, 𝑡]. The 
factor  κ  is  introduced  to  model  the  hysteresis  that  characterizes  this  material  (and 
material 57).  The decay coefficient 𝛽 is introduced to get a reloading curve similar to the 
original loading curve. 
This factor κ is treated as a constant in the determination of the tangent stiffness 
matrix. 
22.121.4  Viscous Stress 
In addition to the hyperelastic stress described above, a viscous stress is added.  
Converting to Voigt notation, this stress can be written 
𝛔 = 𝐂𝐃,
(22.121.14)
where  𝛔  denotes  Cauchy  stress,  𝐃  is  the  rate-of-deformation  and  𝐂  is  an  isotropic 
constitutive  matrix  representing  the  viscosity.    In  element  m,  the  constitutive  matrix 
depends on the element deformation according to 
𝐂 =
𝑑𝑚
𝐂0,
(22.121.15)
where  𝑑𝑚  is  the  diameter5  of  element  m  and  𝐂0  is  a  constitutive  matrix  that  depends 
only  on  the  material  parameters.    Following  material  models  177  and  178  we  use  the 
following material tangent stiffness for this stress contribution 
5 Experiments indicate that d(cid:2923) is the smallest dimension of the element.
LS-DYNA Theory Manual 
Material Models 
𝐂mat =
𝛽Δ𝑡
𝐂,
(22.121.16)
where 𝛾 and 𝛽 are parameters in the Newmark scheme and Δ𝑡 is the time step. 
22.121.5  Viscoelastic Stress Contribution 
An optional viscoelastic stress contribution can be added.  The evolution of this 
stress in time can be stated as 
where 
∇,
∇ = 𝐸d𝑠𝑖𝑗
𝜎𝑖𝑗
∇ = 𝐷𝑖𝑗 − 𝛽1𝑠𝑖𝑗.
𝑠𝑖𝑗
(22.121.17)
(22.121.18)
Here  𝐸d  and  𝛽1  are  material  constants,  𝐷𝑖𝑗  is  the  rate-of-deformation  tensor  and  ∇ 
stands for an objective rate.  Referring to material models 177 and 178, we state that the 
tangent stiffness modulus for this stress contribution can be written 
𝐶𝑖𝑗𝑘𝑙 =
𝐸d
(𝛿𝑖𝑘𝛿𝑗𝑙 + 𝛿𝑖𝑙𝛿𝑗𝑘).
(22.121.19)
This stress acts only in the direction of the principal stretches.  Hence the tangent 
modulus  is  formed  in  the  principal  basis,  modified  to  account  for  this  condition  and 
then transformed back to the global frame of reference. 
22.121.6  Stress Corresponding to First Load Cycle 
We define a contribution to the principal Kirchhoff stress as  
1 𝜏𝑖𝑖
E = 𝜆𝑖{𝑔s(1 − 𝜆𝑖) − 𝑓s(1 − 𝜆𝑖)}𝜉 .
(22.121.20)
When the damage is isotropic the factor 𝜉  is given by 
𝜉 = max (0,1 −
𝜀h
0.0001 + 𝜀m
).
(22.121.21)
where  𝜀h  is  the  damage  parameter  that  is  initially  zero  and  𝜀m  is  the  maximum 
compressive  volumetric  strain  during  the  entire  simulation  thus  far.    Damage  evolves 
when the material is in compression and unloads  
Δ𝜀h = {
max(0, Δ𝐽) otherwise
if  𝐽 ≥ 1
,
(22.121.22)
where  𝐽  is  the  jacobian  of  the  deformation.    The  first  load  cycle  will  result  in  a  total 
stress that follows load curve 𝑔𝑠 since there is no damage.  After a complete load cycle, 
i.e., unloading has occurred, the material is completely damaged, i.e., 𝜀h ≈ 𝜀m, and the
Material Models 
LS-DYNA Theory Manual 
nominal  stress  will  for  the  second  and  subsequent  load  cycles  be  given  by  the  load 
curve 𝑓s. 
In the orthotropic case the principal Kirchhoff stress contribution is instead given 
by 
1 𝜏𝑖𝑖
E = 𝜆𝑖{𝑔𝑠(1 − 𝜆𝑖) − 𝑓𝑠(1 − 𝜆𝑖)}𝜉𝑖.
(22.121.23)
For the damage to be orthotropic we introduce a symmetric and positive definite 
𝑖𝑗. This tensor is initially the zero tensor corresponding to no damage.  
damage tensor 𝜀h
The  evolution  of  damage  begins  with  a  half  step  Jaumann  rotation  of  the  tensor  to 
maintain objectivity.   After that the local increment is performed.  As for the isotropic 
case, damage evolves in compression in combination with unloading.  We introduce the 
local damage increment as 
Δ𝜀loc
if  𝜆𝑖 ≥ 1
𝑖𝑗 = 𝛿𝑖𝑗 {
max(0, Δ𝜆𝑖) otherwise
,
(22.121.24)
which is a diagonal tensor.  The global damage tensor increment is given by 
𝑖𝑗 = 𝑞𝑖𝑘𝑞𝑗𝑙Δ𝜀loc
𝑘𝑙 ,
Δ𝜀ℎ
(22.121.25)
which is used to increment the damage tensor 𝜀ℎ
𝑘𝑙
𝑞𝑘𝑖𝑞𝑙𝑖𝜀ℎ
⎟⎞.
0.0001 + 𝜀m⎠
⎜⎛0,1 −
⎝
𝜉𝑖 = max
𝑖𝑗. The factor 𝜉𝑖 is now given by 
(22.121.26)
where  the  quantity  𝜀m  in  the  orthotropic  case  is  the  maximum  compressive  principal 
strain  in  any  direction  during  the  simulation  thus  far.    As  for  the  isotropic  case,  the 
material  is  completely  damaged  after  one  load  cycle  and  reloading  will  follow  load 
curve 𝑓s. In addition, the directions corresponding to no loading will remain unaffected. 
The factors 𝜉  and 𝜉𝑖 are treated as constants in the determination of the tangent 
stiffness so the contribution is regarded as hyperelastic and follows the exposition given 
in Section 19.179.1. 
The  reason  for  not  differentiating  the  coefficients  𝜅,  𝜉   and  𝜉𝑖  is  that  they  are 
always non-differentiable.  Their changes depend on whether the material is loaded or 
unloaded,  i.e.,  the  direction  of  the  load.    Even  if  they  were  differentiable  their 
contributions would occasionally result in a non-symmetric tangent stiffness matrix and 
any  attempt  to  symmetrize  this  would  probably  destroy  its  properties.    After  all,  we 
believe that the one-dimensional nature and simplicity of this foam will be enough for 
good convergence properties even without differentiating these coefficients.
LS-DYNA Theory Manual 
Material Models 
22.122  Material Model 181:  Simplified Rubber/Foam 
Material  type  181  in  LS-DYNA  is  a  simplified  “quasi”-hyperelastic  rubber  or 
foam model defined by a single uniaxial load curve or by a family of curves at discrete 
strain rates.  The term “quasi” is used because there is really no strain energy function 
for determining the stresses used in this model.  Rather the stress response mimics the 
gradient  of  the  strain  energy  potential  in  the  Ogden  rubber  .    For 
deriving the tangent stiffness matrix we use the formulas as if a strain energy function 
were present, with appropriate modifications. 
This  model  is  equipped  with  various  features  related  to  dissipation  and  damage,  but 
not all of those are described in detail. 
𝐴 
𝑔(𝜆) = 𝑃/𝐴
𝜆 = 𝜆1 = 𝑙/𝐿 
𝜆2 = 𝜆3 = 𝑑/𝐷 
𝐷 
22-122 Uniaxial test parameters. 
22.122.1  Hyperelasticity Using the Principal Stretch Ratios 
A hyperelastic constitutive law is determined by a strain energy function that we 
assume is expressed in terms of the principal stretches, i.e., 𝑊 = 𝑊(𝜆1, 𝜆2, 𝜆3). To obtain 
the  Cauchy  stress  𝜎𝑖𝑗  this  is  first  calculated  in  the  principal  basis  after  which  it  is 
transformed back to the “base frame”, or standard basis.  The complete set of formulas 
is given by Crisfield [1997] and is for the sake of completeness recapitulated here.  For 
the following discussion we refer to figure 22-122 
The principal Kirchhoff stress components are given by 
E = 𝜆𝑖
𝜏𝑖𝑖
𝜕𝑊
𝜕𝜆𝑖
(no sum),
(22.122.1)
that are transformed to the standard basis using the standard formula
Material Models 
LS-DYNA Theory Manual 
E.
𝜏𝑖𝑗 = 𝑞𝑖𝑘𝑞𝑗𝑙𝜏𝑘𝑙
(22.122.2)
The 𝑞𝑖𝑗 are the components of the orthogonal tensor containing the eigenvectors 
of the principal basis.  The Cauchy stress is then given by 
𝜎𝑖𝑗 = 𝐽−1𝜏𝑖𝑗,
(22.122.3)
where 𝐽 = 𝜆1𝜆2𝜆3 is the relative volume change. 
Now, the Ogden strain energy potential results in a Kirchhoff stress on the form 
𝐸 = 𝑓 (𝜆̃𝑖) + 𝐾𝑚(𝐽 − 1) −
𝜏𝑖𝑖
∑ 𝑓 (𝜆̃𝑘)
𝑘=1
(22.4)
for a (large) bulk modulus 𝐾𝑚 and where 𝜆̃𝑖 = 𝜆𝑖/𝐽1/3 are the isochoric stretches.  In the 
Ogden material, 𝑓  has a specific form a priori that requires a least square approximation 
for fitting test data.  This is of course a restriction and the idea in material 181 is to let 𝑓  
be determined directly from input data.  The ansatz for the compressible foam option is 
to let  
𝐸 = 𝑓 (𝜆𝑖) − 𝑓 (𝐽
𝜏𝑖𝑖
− 𝜈
1−2𝜈) 
(22.5)
for a given Poisson’s ratio 𝜈, a decision that will be made clear below.  So assume that 
𝑔(𝜆)  is  the  curve  providing  the  engineering  stress  as  function  of  stretch  in  a  uniaxial 
test, see figure 22-122, then the principal Kirchhoff stresses are 
𝐸 = 𝜆𝑔(𝜆) 
𝜏11
𝐸 = 0
𝐸 = 𝜏33
𝜏22
What  follows  is  the  determination  of  the  internal  function  𝑓   for  the  rubber  and  foam 
option. 
(22.6)
22.122.1.1 
For incompressibility we deduce that the principal stretches are 
 Determination of f, rubber option 
which coincide with the isochoric counterparts.  Using these expressions when equating 
(22.4) and (22.6), one must determine 𝑓  from 
𝜆1 = 𝜆
𝜆2 = 𝜆3 = 𝜆−1/2
(22.7)
(𝑓 (𝜆) − 𝑓 (𝜆−1/2)) + 𝐾𝑚(𝐽 − 1) 
(𝑓 (𝜆−1/2) − 𝑓 (𝜆)) + 𝐾𝑚(𝐽 − 1). 
𝜆𝑔(𝜆) =
0 =
By subtracting these two equations to eliminate the influence of the pressure we get 
(22.8)
that can be rewritten as 
𝜆𝑔(𝜆) = 𝑓 (𝜆) − 𝑓 (𝜆
−1
2) 
𝑓 (𝜆) = 𝜆𝑔(𝜆) + 𝑓 (𝜆−1/2). 
This in turn can be recursively expanded as 
(22.9)
(22.10)
LS-DYNA Theory Manual 
Material Models 
𝑓 (𝜆) = 𝜆𝑔(𝜆) + 𝜆−1/2𝑔(𝜆−1/2) + 𝜆1/4𝑔(𝜆1/4) + ⋯ + 𝑓 (𝜆(−1/2)𝑛
) 
(22.11)
) 
and  by  letting  𝑛  be  large  enough  the  function  𝑓   can  be  determined  since  the  last  term 
tends to zero. 
 Determination of f, foam option 
22.122.1.2 
Similarly, for a given Poisson’s ratio 𝜈, the principal stretches in a uniaxial tension test 
are 
𝜆1 = 𝜆
𝜆2 = 𝜆3 = 𝜆−𝜈
(22.12)
and using (22.5) and (22.6) the equation to solve is now 
(22.13)
Note  that  the  equation  corresponding  to  the  second  of  (22.6)  vanishes  because  of  the 
ansatz  in  (22.5).  The  same  technique  as  for  the  rubber  option  is  used,  recursive 
expansion gives 
𝜆𝑔(𝜆) = 𝑓 (𝜆) − 𝑓 (𝜆−𝜈) 
) + ⋯ + 𝑓 (𝜆(−𝜈)𝑛
which for a large 𝑛 gives a sufficiently accurate representation of 𝑓 . 
𝑓 (𝜆) = 𝜆𝑔(𝜆) + 𝜆−𝜈𝑔(𝜆−𝜈) + 𝜆𝜈2
𝑔(𝜆𝜈2
) 
(22.14)
22.122.2  Some Remarks 
22.122.2.1 
 Strain rates 
The  function  𝑓   introduced  in  the  previous  section  depends  not  only  on  the 
stretches  but  for  some  choices  of  input  also  on  the  strain  rate.    In  this  case  each  test 
curve  𝑔𝑖(𝜆)  corresponding  to  a  particular  strain  rate  𝜀̇𝑖 is  converted  to  an  internal 
function 𝑓𝑖(𝜆) following the procedure described in the previous section.  These internal 
functions  are  then  used  for  determining  the  response  for  a  given  strain  rate  𝜀̇  by 
interpolation.    Strain  rates  are  treated  in  various  ways  depending  on  user  defined 
parameters and we refer to Section and the Keyword Manual for more info. 
22.122.2.2 
 Modeling of the Frequency Independent Damping 
An  elastic-plastic  stress  𝜎𝑑  is  added  to  model  the  frequency  independent 
damping  properties  of  rubber.    This  stress  is  deviatoric  and  determined  by  the  shear 
modulus 𝐺 and the yield stress 𝜎𝑌. This part of the stress is updated incrementally as 
𝑛 + 2𝑮𝑰dev𝛥𝜺,
(22.122.15)
𝑛+1 = 𝝈𝑑
𝝈̃𝑑
where 𝛥𝜺 is the strain increment.  The trial stress is then radially scaled (if necessary) to 
the yield surface according to 
𝑛+1 = 𝜎̃𝑑
𝜎𝑑
𝑛+1min (1,
𝜎𝑌
𝜎eff
),
(22.122.16)
where 𝜎eff is the effective von Mises stress for the trial stress 𝜎̃𝑑
𝑛+1.
Material Models 
LS-DYNA Theory Manual 
22.123  Material Model 187:  Semi-Analytical Model for the 
Simulation of Polymers 
22.123.1  Material law formulation 
 Choice of a yield surface formulation 
All plastics are to some degree anisotropic.  The anisotropic characteristic can be 
due to fibre reinforcement, to the moulding process or it can be load induced in which 
case the material is at least initially isotropic.  Therefore a quadratic form in the stress 
tensor is often used to describe the yield surface.  We restrict the scope of this work to 
isotropic formulations.  However, the choice of this yield surface was made in view of 
later anisotropic generalisations.  In the isotropic case the most general quadratic yield 
surface can be written as 
𝑓 = 𝛔T𝐅𝛔 + 𝐁𝛔 + 𝐹0 ≤ 0,
(22.123.1)
where 
𝛔 =
⎝
⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛
⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛
⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛
⎝
, 
⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞
σ𝑥𝑥
σ𝑦𝑦
σ𝑧𝑧
σ𝑥𝑦
σ𝑦𝑧
σ𝑧𝑥⎠
𝐹11 𝐹12 𝐹12
𝐹12 𝐹11 𝐹12
𝐹12 𝐹12 𝐹11
𝐹1
𝐹1
𝐹1
, 
𝐅 =
⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞
𝐹44
𝐹44⎠
𝐹44
Some  restrictions  apply  to  the  choice  of  the  coefficients.    The  existence  of  a  stress-free 
state  and  the  equivalence  of  pure  shear  and  biaxial  tension/compression  require 
respectively 
0⎠
⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞
𝐁 =
(22.123.2)
⎝
. 
𝐹0 ≤ 0  and 𝐹44 = 2(𝐹11 − 𝐹12).
(22.123.3)
Although  4  independent  coefficients  remain  in  the  expression  for  the  isotropic  yield 
surface  at  this  point,  however  the  yield  condition  is  not  affected  if  all  coefficients  are 
multiplied  by  a  constant.    Consequently  only  3  coefficients  can  be  freely  chosen  and  3 
experiments under different states of stress can be fitted by this formulation.
LS-DYNA Theory Manual 
Material Models 
Figure 22.1.  Recommended tests for material data in SAMP 
Without  loss  of  generality  the  expression  for  the  yield  surface  can  be 
reformulated in terms of the first two stress invariants: pressure and von Mises stress: 
𝑝 = −
σ𝑥𝑥 + σ𝑦𝑦 + σ𝑧𝑧
,
σvm = √
((σ𝑥𝑥 + 𝑝)2 + (σ𝑦𝑦 + 𝑝)
+ (σ𝑧𝑧 + 𝑝)2 + 2σ𝑥𝑦
2 + 2σ𝑦𝑧
2 )
2 + 2σ𝑧𝑥
. 
(22.123.4)
The expression for the yield surface then becomes 
𝑓 = σvm
2 − 𝐴0 − 𝐴1𝑝 − 𝐴2𝑝2 ≤ 0,
(22.123.5)
and identification of the coefficients gives 
𝐴0 = −𝐹0  ,   𝐴1 = 3𝐹1
and 𝐴2 = 9(1 − 𝐹11),
(22.123.6)
or equivalently 
𝐹0 = −𝐴0, 𝐹1 =
𝐴1
, 𝐹11 = 1 −
𝐴2
, 𝐹44 = 3 and 𝐹12 = 𝐹11 −
𝐹44
= − (
+
𝐴2
). 
(22.123.7)
Since  there  is  no  loss  of  generality,  the  simpler  formulation  in  invariants  is  adopted 
from  this  point  on.    In  principle  the  coefficients  of  the  yield  surface  can  now  be 
determined from 3 experiments.  Typically we would perform uniaxial tension, uniaxial 
compression and simple shear tests: 
This allows computation of the coefficients in function of the test results: 
3σs
2 = 𝐴0
2 = 3σs
σt
2 − 𝐴1
2 = 3σs
σc
2 + 𝐴1
σt
σc
+ 𝐴2
+ 𝐴2
⎫
}}}}
σt
}}}}
σc
9 ⎭
⎬
⇒
⎧𝐴0 = 3σs
{{{{
𝐴1 = 9σs
{{{{
𝐴2 = 9 (
⎨
⎩
)
2 (
σc − σt
σcσt
σcσt − 3σs
σcσt
)
. 
(22.123.8)
Alternatively we can also compute the coefficients relating to the formulation in stress 
space:
Material Models 
LS-DYNA Theory Manual 
𝐹1 = 𝐹0 (
−
𝐹0 + 𝐹1𝜎t + 𝐹11σt
2 = 0
𝐹0 − 𝐹1σc + 𝐹11σc
2 = 0
𝐹0 + 𝐹44σs
2 = 0
⎫
}}}}}
}}}}}
⎬
⎭
⇒
⎧
{{{{{
{{{{{
⎨
⎩
𝐹11 = −
𝐹44 = −
σc
𝐹0
σtσc
𝐹0
σs
σt
)
. 
(22.123.9)
Both are easily seen to be equivalent. 
 Conditions for convexity of the yield surface 
Usually the yield surface is required to be convex, i.e. 
𝑓 (σ1) ≤ 0
}⎫
𝑓 (σ2) ≤ 0
0 ≤ α ≤ 1⎭}⎬
   ⇒  𝑓 (ασ1 + (1 − α)σ2) ≤ 0. 
(22.123.10)
The second derivative of 𝑓  is computed as 
𝑓 = 𝛔T𝐅𝛔 + 𝐁𝛔 + 𝐹0 →
∂2𝑓
∂σ2 = 2𝐅
(22.123.11)
A sufficient condition for convexity in 6D stress space is then that the matrix F should 
be  positive  semidefinite.    This  means  all  eigenvalues  of  F  should  be  positive  or  zero.  
The  conditions  for  convexity  will  now  be  examined  in  physical  terms  for  two  cases: 
plane stress and general 3D. 
The plane stress case 
In the plane stress case the yield condition reduces to: 
𝑓 = 𝛔T𝐅𝛔 + 𝐁𝛔 + 𝐹0,
where 
⎟⎞, 
0⎠
And convexity requires the eigenvalues of F to be non-negative: 
𝐹11 𝐹12
𝐹12 𝐹11
𝐹44⎠
⎟⎟⎞   𝐁 =
⎟⎟⎞   𝐅 =
𝐹1
𝐹1
σ𝑥𝑥
σ𝑦𝑦
σ𝑥𝑦⎠
⎜⎜⎛
⎝
⎜⎜⎛
⎝
𝛔 =
⎜⎛
⎝
𝐹11 + 𝐹12 ≥ 0
𝐹11 − 𝐹12 ≥ 0
𝐹44 ≥ 0
}⎫
⎭}⎬
⇒ {
2 ≥ σtσc
4σs
−𝐹0 ≥ 0
. 
(22.123.12)
(22.123.13)
(22.123.14)
The 3D case 
In the full 3D case, the convexity condition is generally more stringent.  Again we 
require the eigenvalues of F to be non-negative, where F is now the full 6 by 6 matrix: 
𝐹11 + 2𝐹12 ≥ 0
𝐹11 − 𝐹12 ≥ 0
𝐹44 ≥ 0
}⎫
⎭}⎬
⇒ {
2 ≥ σtσc
3σs
−𝐹0 ≥ 0
. 
(22.123.15)
LS-DYNA Theory Manual 
Material Models 
Leading to 
σs ≥
√σtσc
√3
>
√σtσc
.
(22.123.16)
Alternatively  a  yield  surface  containing  a  linear  rather  than  a  quadratic  term  was 
implemented in SAMP-1.  
𝑓 = σvm − 𝐴0 − 𝐴1𝑝 − 𝐴2𝑝2 ≤ 0.
(22.123.17)
As  it  will  be  difficult  in  general  to  guarantee  a  reasonable  flow  behaviour  from  three 
independent  measurements  in  shear,  tension  and  compression,  a  simplified  flow  rule 
has  been  implemented  as  the  default  in  SAMP-1.  The  generally  non-associated  flow 
surface is given as: 
𝑔 = σvm
2 + α𝑝2.
This flow rule is associated if: 
𝐴1 = 0,
𝐴2 = −α
And clearly leads to a constant value for the plastic Poisson ratio: 
(= cte).
ν𝑝 =
9 − 2α
18 + 2α
⇒ α =
1 − 2ν𝑝
1 + ν𝑝
.
Plausible flow behaviour just means that: 
0 ≤ α ≤
⇒ 0 ≤ ν𝑝 ≤ 0.5.
(22.123.18)
(22.123.19)
(22.123.20)
(22.123.21)
In  SAMP-1  the  value  of  the  plastic  Poisson  coefficient  is  given  by  the  user,  either  as  a 
constant  or  as  a  load  curve  in  function  of  the  uniaxial  plastic  strain.    This  allows 
adjusting  the  flow  rule  of  the  material  to  measurements  of  transversal  deformation 
during uniaxial tensile or compressive testing.  This can be important for plastics since 
often a non-isochoric behaviour is measured.
Material Models 
LS-DYNA Theory Manual 
Figure 22.2.  Influence of the flow rule on the plastic Poisson ratio 
The possible values for the plastic Poisson ratio and the resulting flow behaviour 
are illustrated in Figure 22.2. 
In  SAMP-1  the  formulation  is  slightly  modified  and  based  on  a  flow  rule  given 
as: 
The plastic strain rate computation is not normalized: 
𝑔′ = √σvm
2 + α𝑝2.
ε̇p = λ̇
∂𝑔′
∂σ
.
The volumetric and deviatoric plastic strain rates in this case are given as : 
ε̇vp = λ̇ (−2α𝑝) 2𝑔′⁄
=
ε̇dp = λ̇ 3s 2𝑔′⁄
=
λ̇ (−2α𝑝)
,
2 + 4α𝑝2
√4σvm
λ̇ 3s
, 
√4σvm
2 + 4α𝑝2
(22.123.22)
(22.123.23)
(22.123.24)
which  amounts  to  a  different  definition  of  the  plastic  consistency  parameter  which  of 
course has to be considered when equivalent plastic strain values are computed. 
22.123.2  Hardening formulation 
The hardening formulation is the attractive part of SAMP-1.  The formulation is 
fully tabulated and consequently the user can directly input measurement results from 
uniaxial  tension,  uniaxial  compression  and  simple  shear  tests  in  terms  of  load  curves 
giving  the  yield  stress  as  a  function  of  the  corresponding  plastic  strain.    No  fitting  of 
coefficients is required.  The test results that are reflected in the load curves will be used 
exactly  by  SAMP-1  without  fitting  to  any  analytical  expression.    Consequently  the
LS-DYNA Theory Manual 
Material Models 
Figure 22.3.  Tensile hardening curve from dynamic tensile tests 
hardening  will  be  dependent  upon  the  state  of  stress  and  not  only  upon  the  plastic 
strain. 
22.123.3  Rate effects 
Plastics  are  usually  highly  rate  dependent.    A  proper  viscoplastic  consideration 
of the rate effects is therefore important in the numerical treatment of the material law.  
Data  to  determine  the  rate  dependency  are  based  on  uniaxial  dynamic  testing.    If 
dynamic  tests  are  available,  then  the  load  curve  defining  the  yield  stress  in  uniaxial 
tension  is  simply  replaced  by  a  table  definition  containing  multiple  load  curves 
corresponding  to  different  values  of  the  plastic  strain  rate.    This  is  illustrated  in  the 
Figure 22.3. 
22.123.4  Damage and failure 
Numerous damage models can be found in the literature.  Probably the simplest 
concept  is  elastic  damage  where  the  damage  parameter  (usually  written  as  𝑑)  is  a 
function of the elastic energy and effectively reduces the elastic modulus of the material.  
In  the  case  of  ductile  damage,  𝑑  is  a  function  of  plastic  straining  and  affects  the  yield 
stress rather than the elastic modulus.  This is equivalent to plastic softening.  In more 
sophisticated  damage  models,  d  depends  on  both  the  plastic  straining  and  the  elastic 
energy (and maybe other factors) and effects yield stress as well as elastic modulus. 
A  simple  damage  model  was  added  to  the  SAMP-1  material  law  where  the 
damage parameter d is a function of plastic strain only.  A load curve must be provided 
by the user giving d as a function of the (true) plastic strain under uniaxial tension.  The 
value  of  the  critical  damage  Dc  leading  to  rupture  is  then  the  only  other  required 
additional input.  The implemented damage model is isotropic.
Material Models 
LS-DYNA Theory Manual 
Figure 22.4.  Damage parameter from uniaxial tensile test 
The implemented model then uses the notion of effective cross section, which is 
the true cross section of the material minus the cracks that have developed.  We will use 
the following notation: 
𝐴0 → undeformed cross section 
𝐴  → deformed or current cross section 
𝐴0 → undeformed cross section 
We define the effective stress as the force divided by the effective cross section: 
σ =
σeff =
,
𝐴eff
=
𝐴(1 − 𝑑)
=
1 − 𝑑
,
which allows defining an effective yield stress: 
σy,eff =
σy
1 − 𝑑
.
(22.25)
(22.26)
LS-DYNA Theory Manual 
Material Models 
22.124  Material Model 196:  General Spring Discrete Beam 
If  TYPE = 0,  elastic  behavior  is  obtained.    In  this  case,  if  the  linear  spring 
stiffness is used, the force, 𝐹, is given by: 
𝐹 = 𝐹0 + 𝐾Δ𝐿 + 𝐷Δ𝐿̇,
(22.124.1)
but if the load curve ID is specified, the force is then given by: 
𝐹 = 𝐹0 + 𝐾 𝑓 (Δ𝐿) [1 + 𝐶1 ⋅ Δ𝐿̇ + 𝐶2 ⋅ sgn(Δ𝐿̇)ln (max {1. ,
+ 𝑔(Δ𝐿)ℎ(Δ𝐿̇). 
∣Δ𝐿̇∣
𝐷𝐿𝐸
})] + 𝐷Δ𝐿̇
(22.124.2)
In these equations, Δ𝐿 is the change in length  
Δ𝐿 = current length − initial length.
(22.124.3)
If TYPE = 1, inelastic behavior is obtained.  In this case, the yield force is taken 
from the load curve: 
𝐹Y = 𝐹y(Δ𝐿plastic),
where 𝐿plastic is the plastic deflection.  A trial force is computed as: 
and is checked against the yield force to determine F: 
𝐹T = 𝐹n + KΔ𝐿̇Δ𝑡,
𝐹 = {𝐹Y if 𝐹T > 𝐹Y
𝐹T if 𝐹T ≤ 𝐹Y.
(22.124.4)
(22.124.5)
(22.124.6)
The final force, which includes rate effects and damping, is given by: 
𝐹𝑛+1 = 𝐹 ⋅ [1 + 𝐶1 ⋅ Δ𝐿̇ + 𝐶2 ⋅ sgn(Δ𝐿̇)ln (max {1. ,
+ 𝑔(Δ𝐿)ℎ(Δ𝐿̇).
∣Δ𝐿̇∣
𝐷𝐿𝐸
})] + 𝐷Δ𝐿̇
(22.124.7)
Unless  the  origin  of  the  curve  starts  at  (0,0),  the  negative  part  of  the  curve  is  used 
when  the  spring  force  is  negative  where  the  negative  of  the  plastic  displacement  is 
used to interpolate, 𝐹y.  The positive part of the curve is used whenever the force is 
positive.  
The  cross  sectional  area  is  defined  on  the  section  card  for  the  discrete  beam 
elements, See *SECTION_BEAM.  The square root of this area is used as the contact 
thickness offset if these elements are included in the contact treatment.
LS-DYNA Theory Manual 
Equation of State Models 
23    
Equation of State Models 
LS-DYNA has 10 equation of state models which are described in this section. 
1. 
2. 
3. 
4. 
5. 
6. 
7. 
8. 
9. 
10. 
Linear Polynomial 
JWL High Explosive 
Sack “Tuesday” High Explosive 
Gruneisen 
Ratio of Polynomials 
Linear Polynomial With Energy Deposition 
Ignition and Growth of Reaction in High Explosives 
Tabulated Compaction 
Tabulated 
Propellant-Deflagration 
The  forms  of  the  first  five  equations  of  state  are  given  in  the  KOVEC  user’s 
manual [Woodruff 1973] as well as below. 
23.1  Equation of State Form 1:  Linear Polynomial 
This  polynomial  equation  of  state,  linear  in  the  internal  energy  per  initial 
volume, 𝐸, is given by 
𝑝 = 𝐶0 + 𝐶1𝜇 + 𝐶2𝜇2 + 𝐶3𝜇3 + (𝐶4 + 𝐶5𝜇 + 𝐶6𝜇2)𝐸
Here 𝐶0, 𝐶1, 𝐶2, 𝐶3, 𝐶4, 𝐶5 and 𝐶6 are user defined constants and  
𝜇 =
− 1.
(23.1.1)
(23.1.2)
where 𝑉 is the relative volume.  In expanded elements, the coefficients of 𝜇2 are set to 
zero, i.e., 
𝐶2 = 𝐶6 = 0.
(23.1.3)
Equation of State Models 
LS-DYNA Theory Manual 
The  linear  polynomial  equation  of  state  may  be  used  to  model  gas  with  the 
gamma law equation of state.  This may be achieved by setting: 
and 
𝐶0 = 𝐶1 = 𝐶2 = 𝐶3 = 𝐶6 = 0,
𝐶4 = 𝐶5 = 𝛾 − 1,
where 𝛾 is the ratio of specific heats.  The pressure is then given by: 
Note that the units of 𝐸 are the units of pressure. 
𝑝 = (𝛾 − 1)
𝜌0
𝐸.
(23.1.4)
(23.1.5)
(23.1.6)
23.2  Equation of State Form 2:  JWL High Explosive 
The  JWL  equation  of  state  defines  pressure  as  a  function  of  relative volume,  𝑉, 
and internal energy per initial volume, 𝐸, as 
𝑝 = 𝐴 (1 −
𝑅 1𝑉
) 𝑒−𝑅 1𝑉 + 𝐵 (1 −
𝑅 2𝑉
) 𝑒−𝑅 2𝑉 +
𝜔𝐸
,
(23.2.7)
where 𝜔, A, 𝐵, 𝑅1 and 𝑅2 are user defined input parameters.  The JWL equation of state 
is  used  for  determining  the  pressure  of  the  detonation  products  of  high  explosives  in 
applications involving metal accelerations.  Input parameters for this equation are given 
by Dobratz [1981] for a variety of high explosive materials. 
This equation of state is used with the explosive burn (material model 8) material 
model which determines the lighting time for the explosive element. 
23.3  Equation of State Form 3:  Sack “Tuesday” High 
Explosives 
Pressure of detonation products is given in terms of the relative volume, 𝑉, and 
internal energy per initial volume, 𝐸, as [Woodruff 1973]: 
𝐴 3
𝑉 𝐴1
where 𝐴1, 𝐴2, 𝐴3, 𝐵1 and 𝐵2 are user-defined input parameters. 
𝑒−𝐴 2𝑉 (1 −
𝐵1
𝐵2
) +
𝑝 =
𝐸,
(23.3.8)
LS-DYNA Theory Manual 
Equation of State Models 
This equation of state is used with the explosive burn (material model 8) material 
model which determines the lighting time for the explosive element. 
23.4  Equation of State Form 4:  Gruneisen 
The  Gruneisen  equation  of  state  with  cubic  shock  velocity-particle  velocity 
defines pressure for compressed material as 
)𝜇 − 𝑎
𝜌0𝐶2𝜇[1 + (1 −
𝜇 2]
𝑝 =
𝛾0
𝜇 2
𝜇 + 1
− 𝑆3
𝜇 3
(𝜇 + 1)2]
[1 − (𝑆1 − 1)𝜇 − 𝑆2
2   + (𝛾0 + 𝛼𝜇)𝐸, 
(23.4.9)
where 𝐸 is the internal energy per initial volume, 𝐶 is the intercept of the 𝑢s − 𝑢p curve, 
𝑆1, 𝑆2, and 𝑆3 are the coefficients  of the slope of the 𝑢s − 𝑢p curve, 𝛾0 is the Gruneisen 
gamma, and a is the first order volume correction to 𝛾0.  Constants 𝐶, 𝑆1, 𝑆2, 𝑆3,  𝛾0 and 
𝑎 are user defined input parameters.  The compression is defined in terms of the relative 
volume, 𝑉, as: 
𝜇 =
− 1.
For expanded materials as the pressure is defined by:  
𝑝 = 𝜌0 𝐶 2𝜇 + (𝛾0 + 𝛼𝜇)𝐸.
23.5  Equation of State Form 5:  Ratio of Polynomials 
The ratio of polynomials equation of state defines the pressure as 
𝑝 =
𝐹1 + 𝐹2𝐸 + 𝐹3𝐸2 + 𝐹4𝐸3
𝐹5 + 𝐹6𝐸 + 𝐹7𝐸2
(1 + 𝛼𝜇),
where 
𝐹𝑖 = ∑ 𝐴𝑖𝑗𝑚𝑗
𝑗= 0
,
𝑛 = 4 if 𝑖 < 3,
𝑛 = 3 if 𝑖 ≥ 3
𝜇 =
𝜌0 − 1
.
(23.4.10)
(23.4.11)
(23.5.12)
(23.5.13)
(23.5.14)
Equation of State Models 
LS-DYNA Theory Manual 
In  expanded  zoned  𝐹1  is  replaced  by  𝐹′1 = 𝐹1 + 𝛽𝜇2  Constants  𝐴𝑖𝑗,  𝛼,  and  𝛽  are 
user input. 
23.6  Equation of State Form 6:  Linear With Energy 
Deposition 
This  polynomial  equation  of  state,  linear  in  the  internal  energy  per  initial 
volume, 𝐸, is given by 
𝑝 = 𝐶0 + 𝐶1𝜇 + 𝐶2𝜇2 + 𝐶3𝜇3 + (𝐶4 + 𝐶5𝜇 + 𝐶6𝜇2)𝐸,
Here 𝐶0, 𝐶1, 𝐶2, 𝐶3, 𝐶4, 𝐶5  and 𝐶6 are user defined constants and  
𝜇 =
− 1,
(23.6.15)
(23.6.16)
where 𝑉 is the relative volume.  In expanded elements, we set the coefficients of 𝜇2 to 
zero, i.e., 
𝐶2 = 𝐶6 = 0.
(23.6.17)
Internal  energy,  𝐸,  is  increased  according  to  an  energy  deposition  rate  versus 
time curve whose ID is defined in the input. 
23.7  Equation of State Form 7:  Ignition and Growth Model 
A JWL equation of state defines the pressure in the unreacted high explosive as 
𝑃𝑒 = 𝐴𝑒 (1 −
𝜔𝑒
𝑅1𝑒𝑉𝑒
) 𝑒−𝑅1𝑒𝑉𝑒 + 𝐵𝑒 (1 −
𝜔𝑒
𝑅2 𝑒𝑉𝑒
) 𝑒−𝑅2 𝑒𝑉𝑒 +
𝜔𝑒𝐸
𝑉𝑒
, 
(23.7.18)
where 𝑉𝑒 is the relative volume, 𝐸𝑒 is the internal energy, and the constants 𝐴𝑒, 𝐵𝑒, 𝜔𝑒, 
𝑅1𝑒  and  𝑅2𝑒  are  input  constants.    Similarly,  the  pressure  in  the  reaction  products  is 
defined by another JWL form 
𝑃𝑝 = 𝐴𝑝 (1 −
𝜔𝑝
𝑅1𝑝  𝑉𝑝
) 𝑒−𝑅1𝑝𝑉𝑝 + 𝐵𝑝 (1 −
𝜔𝑒
𝑅2 𝑝𝑉𝑝
) 𝑒−𝑅2 𝑝 𝑉𝑝 +
𝜔 𝑝𝐸
. 
𝑉𝑝
(23.7.19)
The  mixture  of  unreacted  explosive  and  reaction  products  is  defined  by  the 
fraction  reacted  𝐹  (𝐹 = 0  implies  no  reaction,  𝐹 = 1  implies  complete  conversion  from 
explosive  to  products).    The  pressures  and  temperature  are  assumed  to  be  in 
equilibrium, and the relative volumes are assumed to be additive:
LS-DYNA Theory Manual 
Equation of State Models 
𝑉 = (1 − 𝐹)𝑉𝑒 + 𝐹𝑉𝑝.
(23.7.20)
The rate of reaction is defined as 
=  𝐼(FCRIT − 𝐹)𝑦(𝑉𝑒
∂𝐹
∂𝑡
where 𝐼, 𝐺, 𝐻, 𝑥, 𝑦, 𝑧 and 𝑚 (generally 𝑚 = 0) are input constants. 
−1 − 1)] + 𝐻(1 − 𝐹)𝑦𝐹𝑥𝑃𝑧(𝑉𝑝
[1 + 𝐺(𝑉 𝑒
−1 − 1)
−1 − 1)
,
(23.7.21)
The  JWL  equations  of  state  and  the  reaction  rates  have  been  fitted  to  one-  and 
two-dimensional  shock  initiation  and  detonation  data  for  four  explosives:    PBX-9404, 
RX-03-BB,  PETN,  and  cast  TNT.    The  details  of  calculational  method  are  described  by 
Cochran  and  Chan  [1979].    The  detailed  one-dimensional  calculations  and  parameters 
for  the  four  explosives  are  given  by  Lee  and  Tarver  [1980].    Two-dimensional 
calculations  with  this  model  for  PBX  9404  and  LX-17  are  discussed  by  Tarver  and 
Hallquist [1981]. 
23.8  Equation of State Form 8:  Tabulated Compaction 
Pressure  is  positive  in  compression,  and  volumetric  strain  𝜀𝑉  is  positive  in 
tension.  The tabulated compaction model is linear in internal energy per unit volume.  
Pressure is defined by 
𝑝 = 𝐶(𝜀𝑉) + 𝛾𝑇(𝜀𝑉)𝐸,
(23.8.22)
during  loading (compression).   Unloading  occurs at a slope corresponding  to  the bulk 
modulus  at  the  peak  (most  compressive)  volumetric  strain,  as  shown  in  Figure  23.1.  
Reloading  follows  the  unloading  path  to  the  point  where  unloading  began,  and  then 
continues on the loading path described by Equation (23.8.22). 
23.9  Equation of State Form 9:  Tabulated 
The  tabulated  equation  of  state  model  is  linear  in  internal  energy.    Pressure  is 
defined by 
𝑝 = 𝐶(𝜀𝑉) + 𝛾𝑇(𝜀𝑉)𝐸,
(23.9.23)
The volumetric strain 𝜀𝑉 is given by the natural algorithm of the relative volume.  Up to 
10  points  and  as  few  as  2  may  be  used  when  defining  the  tabulated  functions.    The 
pressure is extrapolated if necessary.  Loading and unloading are along the same curve 
unlike equation of state form 8.
Equation of State Models 
LS-DYNA Theory Manual 
kεA
εA
kεC
εC
V)
kεB
εB
(-ε
Volumetric Strain
Figure 23.1.  Pressure versus volumetric strain curve for equation of state form 
8  with  compaction.    In  the  compacted  states,  the  bulk  unloading  modulus
depends on the peak volumetric strain. 
23.10  Equation of State Form 10:  Propellant-Deflagration 
A  deflagration  (burn  rate)  reactive  flow  model  requires  an  unreacted  solid 
equation-of-state, a reaction product equation-of-state, a reaction rate law and a mixture 
rule  for  the  two  (or  more)  species.    The  mixture  rule  for  the  standard  ignition  and 
growth model [Lee and Tarver 1980] assumes that both pressures and temperatures are 
completely  equilibrated  as  the  reaction  proceeds.    However,  the  mixture  rule  can  be 
modified to allow no thermal conduction or partial heating of the solid by the reaction 
product  gases.    For  this  relatively  slow  process  of  airbag  propellant  burn,  the  thermal 
and pressure equilibrium assumptions are valid.  The equations-of-state currently used 
in  the  burn  model  are  the  JWL,  Gruneisen,  the  van  der  Waals  co-volume,  and  the 
perfect  gas  law,  but  other  equations-of-state  can  be  easily  implemented.    In  this 
propellant burn, the gaseous nitrogen produced by the burning sodium azide obeys the 
perfect gas law as it fills the airbag but may have to be modeled as a van der Waal’s gas 
at  the  high  pressures  and  temperatures  produced  in  the  propellant  chamber.    The 
chemical reaction rate law is pressure, particle geometry and surface area dependant, as 
are  most  high-pressure  burn  processes.    When  the  temperature  profile  of  the  reacting 
system is well known, temperature dependent Arrhenius chemical kinetics can be used. 
Since  the  airbag  propellant  composition  and  performance  data  are  company 
private information, it is very difficult  to obtain the required information for burn rate 
modeling.  However, Imperial Chemical Industries (ICI) Corporation supplied pressure
LS-DYNA Theory Manual 
Equation of State Models 
exponent,  particle  geometry,  packing  density,  heat  of  reaction,  and  atmospheric 
pressure  burn  rate  data  which  allowed  us  to  develop  the  numerical  model  presented 
here  for  their  NaN3 + Fe2O3  driver  airbag  propellant.    The  deflagration  model,  its 
implementation, and the results for the ICI propellant are presented in the are described 
by [Hallquist, et.  al., 1990].  
The unreacted propellant and the reaction product equations-of-state are both of 
the form: 
𝑝 = 𝐴 𝑒−𝑅1𝑉 + 𝐵𝑒−𝑅2𝑉 +
𝜔𝐶v𝑇
𝑉 − 𝑑
,
(23.10.24)
where  𝑝  is  pressure  (in  Mbars),  𝑉  is  the  relative  specific  volume  (inverse  of  relative 
density),  𝜔  is  the  Gruneisen  coefficient,  𝐶v  is  heat  capacity  (in  Mbars  -cc/cc°K),  𝑇  is 
temperature in °𝐾, 𝑑 is the co-volume, and 𝐴, 𝐵, 𝑅1 and 𝑅2 are constants.  Setting 𝐴 =
𝐵 = 0 yields the van der Waal’s co-volume equation-of-state.  The JWL equation-of-state 
is  generally  useful  at  pressures  above  several  kilobars,  while  the  van  der  Waal’s  is 
useful at pressures below that range and above the range for which the perfect gas law 
holds.  Of course, setting 𝐴 = 𝐵 = 𝑑 = 0 yields the perfect gas law.  If accurate values of 
𝜔  and  𝐶v  plus  the  correct  distribution  between  “cold”  compression  and  internal 
energies are used, the calculated temperatures are very reasonable and thus can be used 
to check propellant performance. 
The reaction rate used for the propellant deflagration process is of the form: 
= 𝑍(1 − 𝐹)𝑦 𝐹𝑥 𝑝𝑤 + 𝑉(1 − 𝐹)𝑢 𝐹𝑟𝑝𝑠
∂𝐹
∂𝑡
for  0 < 𝐹 < 𝐹limit1 
for  𝐹limit2 < 𝐹 < 1
(23.10.25)
where 𝐹 is the fraction reacted (𝐹 = 0 implies no reaction, 𝐹 = 1 is complete reaction), 𝑡 
is time, and 𝑝 is pressure (in Mbars), 𝑟, 𝑠, 𝑢, 𝑤, 𝑥, 𝑦,  𝐹limit1 and 𝐹limit2 are constants used 
to describe the pressure dependence and surface area dependence of the reaction rates.  
Two (or more) pressure dependent reaction rates are included in case the propellant is a 
mixture  or  exhibited  a  sharp  change  in  reaction  rate  at  some  pressure  or temperature.  
Burning  surface  area  dependences  can  be  approximated  using  the  (1 − 𝐹)𝑦𝐹𝑥  terms.  
Other forms of the reaction rate law, such as Arrhenius temperature dependent 𝑒−𝐸/𝑅𝑇 
type  rates,  can  be  used,  but  these  require  very  accurate  temperatures  calculations.  
Although  the  theoretical  justification  of  pressure  dependent  burn  rates  at  kilobar  type 
pressures is not complete, a vast amount of experimental burn rate versus pressure data 
does demonstrate this effect and hydrodynamic calculations using pressure dependent 
burn accurately simulate such experiments. 
The  deflagration  reactive  flow  model  is  activated  by  any  pressure  or  particle 
velocity  increase  on  one  or  more  zone  boundaries  in  the  reactive  material.    Such  an 
increase creates pressure in those zones and the decomposition begins.  If the pressure 
is relieved, the reaction rate decreases and can go to zero.  This feature is important for
Equation of State Models 
LS-DYNA Theory Manual 
short  duration,  partial  decomposition  reactions.    If  the  pressure  is  maintained,  the 
fraction  reacted  eventually  reaches  one  and  the  material  is  completely  converted  to 
product  molecules.    The  deflagration  front  rates  of  advance  through  the  propellant 
calculated  by  this  model  for  several  propellants  are  quite  close  to  the  experimentally 
observed burn rate versus pressure curves. 
To  obtain  good  agreement  with  experimental  deflagration  data,  the  model 
requires an accurate description of the unreacted propellant equation-of-state, either an 
analytical  fit  to  experimental  compression  data  or  an  estimated  fit  based  on  previous 
experience with similar materials.  This is also true for the reaction products equation-
of-state.    The  more  experimental  burn  rate,  pressure  production  and  energy  delivery 
data  available,  the  better  the  form  and  constants  in  the  reaction  rate  equation  can  be 
determined. 
Therefore  the  equations  used  in  the  burn  subroutine  for  the  pressure  in  the 
unreacted propellant 
  𝑃𝑢 = 𝑅1 ⋅ 𝑒−𝑅5⋅𝑉𝑢 + 𝑅2 ⋅ 𝑒−𝑅6⋅𝑉𝑢 +
𝑅3 ⋅ 𝑇𝑢
𝑉𝑢 − FRER
,
(23.10.26)
where 𝑉𝑢 and 𝑇𝑢 are the relative volume and temperature respectively of the unreacted 
propellant.    The  relative  density  is  obviously  the  inverse  of  the  relative  volume.    The 
pressure 𝑃p in the reaction products is given by: 
𝑃p =  𝐴 ⋅ 𝑒−𝑋𝑃1⋅𝑉𝑝 + 𝐵 ⋅ 𝑒−𝑋𝑃2⋅𝑉𝑝 +
𝐺 ⋅ 𝑇𝑝
𝑉𝑝 − CCRIT
.
(23.10.27)
As  the  reaction  proceeds,  the  unreacted  and  product  pressures  and  temperatures  are 
assumed  to  be  equilibrated  (𝑇𝑢 = 𝑇𝑝 = 𝑇, 𝑝 = 𝑃𝑢 = 𝑃𝑝)  and  the  relative  volumes  are 
additive: 
𝑉 = (1 − 𝐹) ⋅ 𝑉𝑢 + 𝐹 ⋅ 𝑉𝑝
(23.10.28)
where  𝑉  is  the  total  relative  volume.    Other  mixture  assumptions  can  and  have  been 
used in different versions of DYNA2D/3D.  The reaction rate law has the form: 
= GROW1(𝑝 + FREQ)𝑒𝑚(𝐹 + FMXIG)𝑎𝑟1(1 − 𝐹 + FMXIG)𝑒𝑠1
∂𝐹
∂𝑡
+GROW2(𝑝 + FREQ)𝑒𝑛(𝐹 + FMXIG)
(23.10.29)
If  𝐹  exceeds  FMXGR,  the  GROW1  term  is  set  equal  to  zero,  and,  if  𝐹  is  less 
thanFMNGR, the GROW2 term is zero.  Thus, two separate (or overlapping) burn rates 
can be used to describe the rate at which the propellant decomposes. 
This  equation-of-state  subroutine  is  used  together  with  a  material  model  to 
describe the propellant.  In the airbag propellant case, a null material model (type #10) 
can be used.  Material type #10 is usually used for a solid propellant or explosive when 
the shear modulus and yield strength are defined.  The propellant material is defined by
LS-DYNA Theory Manual 
Equation of State Models 
the  material  model  and  the  unreacted  equation-of-state  until  the  reaction  begins.    The 
calculated  mixture  states  are  used  until  the  reaction  is  complete  and  then  the  reaction 
product  equation-of-state  is  used.    The  heat  of  reaction,  ENQ,  is  assumed  to  be  a 
constant and the same at all values of 𝐹 but more complex energy release laws could be 
implemented.
LS-DYNA Theory Manual 
Artificial Bulk Viscosity 
24    
Artificial Bulk Viscosity 
Bulk viscosity is used  to treat shock waves.  Proposed in one spatial dimension 
by  von  Neumann  and  Richtmyer  [1950],  the  bulk  viscosity  method  is  now  used  in 
nearly all wave propagation codes.  A viscous term 𝑞 is added to the pressure to smear 
the shock discontinuities into rapidly varying but continuous transition regions.  With 
this  method  the  solution  is  unperturbed  away  from  a  shock,  the  Hugoniot  jump 
conditions  remain  valid  across  the  shock  transition,  and  shocks  are  treated 
automatically.    In  our  discussion  of  bulk  viscosity  we  draw  heavily  on  works  by 
Richtmyer  and  Morton  [1967],  Noh  [1976],  and  Wilkins  [1980].    The  following 
discussion  of  the  bulk  viscosity  applies  to  solid  elements  since  strong  shocks  are  not 
normally encountered in structures modeled with shell and beam elements. 
24.1  Shock Waves 
Shock waves result from the property that sound speed increases with increasing 
pressure.    A  smooth  pressure  wave  can  gradually  steepen  until  it  propagates  as  a 
discontinuous  disturbance  called  a  shock.    See  Figure  24.1.    Shocks  lead  to  jumps  in 
pressure, density, particle velocity, and energy. 
Consider a planar shock front moving through a material.  The velocity ahead of 
the  shock  is  𝑢1;  the  velocity  behind  is  𝑢2;  and  the  shock  velocity  is  𝑢𝑠.    Mass, 
momentum,  and  energy  are  conserved  across  the  front.    Application  of  these 
conservation laws leads to the well-known Rankine-Hugoniot jump conditions 
(𝜌2 − 𝜌1)𝑢𝑠 = 𝜌2𝑢2 − 𝜌1𝑢1
𝜌2(𝑢𝑠 − 𝑢2)𝑢2 + 𝜌1(𝑢1 − 𝑢𝑠)𝑢1 = 𝑝2 − 𝑝1
(𝐸2 − 𝐸1)𝑢𝑠 = (𝐸2 + 𝑝2)𝑢2 − (𝐸1 + 𝑝1)𝑢1
(24.1)
(24.2)
(24.3)
where Equation (24.3) is an expression of the energy jump condition using the results of 
mass  conservation,  Equation  (24.1),  and  momentum  conservation,  Equation  (24.2).
Artificial Bulk Viscosity 
LS-DYNA Theory Manual 
Figure 24.1.  If the sound speed increases as the stress increases the traveling 
wave above will gradually steepen as it moves along the x-coordinate to form a 
shock wave. 
Here, 𝜌𝑖 is the density, 𝐸𝑖 is the energy density, and 𝑝𝑖 is the pressure; the subscript, 𝑖, is 
1 for ahead of the shock and 2 for behind the shock. 
The  energy  equation  relating  the  thermodynamic  quantities  density,  pressure, 
and energy must be satisfied for all shocks.  The equation of state 
𝑝 = 𝑝(𝜌, 𝑒),
(24.4)
which  defines  all  equilibrium  states  that  can  exist  in  a  material  and  relating  the  same 
quantities as the energy equation, must also be satisfied.  We may use this equation to 
eliminate  energy  from  Equation  (24.3)  and  obtain  a  unique  relationship  between 
pressure and compression.  This relation, called the Hugoniot, determines all pressure-
compression  states  achievable  behind  the  shock.    Shocking  takes  place  along  the 
Rayleigh  line  and  not  the  Hugoniot  (Figure  24.1)  and  because  the  Hugoniot  curve 
closely  approximates  an  isentrope,  we  may  often  assume  the  unloading  follows  the 
Hugoniot.  Combining Equations (24.1) and (24.2) and choosing a coordinate fram such 
that 𝑢1 = 0, we see that the slope of the Rayleigh line is related to the shock speed: 
𝑢𝑠 =
𝜌1
√𝑝2 − 𝑝1
√√
− 1
𝜌2
𝜌1
⎷
.
For the material of Figure 24.2, increasing pressure increases shock speed. 
Consider a 𝛾-law gas with the equation of state 
𝑝 = (𝛾 − 1)𝜌𝑒,
(24.5)
(24.6)
LS-DYNA Theory Manual 
Artificial Bulk Viscosity 
p1
p0
Figure 24.2.  Shocking takes place along the Rayleigh line, and release closely
follows  the  Hugoniot.    The  cross-hatched  area  is  the  difference  between  the 
internal energy behind the shock and the internal energy lost on release. 
where  𝛾  is  the  ratio  of  specific  heats.    Using  the  energy  jump  condition,  we  can 
eliminate 𝑒 and obtain the Hugoniot 
𝑝0
= 𝑝∗ =
2𝑉0 + (𝛾 − 1)(𝑉0 − 𝑉)
2𝑉 − (𝛾 − 1)(𝑉0 − 𝑉)
,
(24.7)
where 𝑉 is the relative volume.  Figure 24.3 shows a plot of the Hugoniot and adiabat 
where it is noted that for 𝑝∗ = 1, the slopes are equal.  Thus for weak shocks, Hugoniot 
and  adiabat  agree  to  the  first  order  and  can  be  ignored  in  numerical  calculations.  
However, special treatment is required for strong shocks, and in numerical calculations 
this special treatment takes the form of bulk viscosity. 
24.2  Bulk Viscosity 
In  the  presence  of  shocks,  the  governing  partial  differential  equations  can  give 
multiple weak solutions.  In their discussion of the Rankine-Hugoniot jump conditions, 
Richtmyer  and  Morton  [1967]  report  that  the  unmodified  finite  difference  (element) 
equations  often  will  not  produce  even  approximately  correct  answers.    One  possible 
solution is to employ shock fitting techniques and treat the shocks as interior boundary 
conditions.  This technique has been used in one spatial dimension but is too complex to 
extend  to  multi-dimensional  problems  of  arbitrary  geometry.    For  these  reasons  the 
pseudo-viscosity method was a major breakthrough for computational mechanics.
Artificial Bulk Viscosity 
LS-DYNA Theory Manual 
Limiting compression
Hugoniot
Adiabat
Slopes of Hugoniot and adiabat
are equat at 
  Figure 24.3.  Hugoniot curve and adiabat for a g-law gas (from [Noh 1976]). 
The  viscosity  proposed  by  von  Neumann  and  Richtmyer  [1950]  in  one  spatial 
dimension has the form  
𝑞 = 𝐶0𝜌(Δ𝑥)2 (
)
∂𝑥̇
∂𝑥
𝑞 = 0
if
if
∂𝑥̇
∂𝑥
∂𝑥̇
∂𝑥
< 0
≥ 0
(24.8)
where  𝐶0  is  a  dimensionless  constant  and  𝑞  is  added  to  the  pressure  in  both  the 
momentum  and  energy  equations.    When  𝑞  is  used,  they  proved  the  following  for 
steady  state  shocks: 
the  hydrodynamic  equations  possess  solutions  without 
discontinuities;  the  shock  thickness  is  independent  of  shock  strength  and  of  the  same 
order  as  the  Δ𝑥  used  in  the  calculations;  the  q  term  is  insignificant  outside  the  shock 
layer; and the jump conditions are satisfied.  According to Noh, it is generally believed 
that these properties: “hold for all shocks, and this has been borne out over the years by 
countless numerical experiments in which excellent agreement has been obtained either 
with exact solutions or with hydrodynamical experiments.” 
In 1955, Landshoff [1955] suggested the addition of a linear term to the 𝑞 of von 
Neumann and Richtmyer leading to a 𝑞 of the form 
𝑞 = 𝐶0𝜌(Δ𝑥)2 (
𝑞 = 𝐶0𝜌(Δ𝑥)2 (
)
)
𝜕𝑥̇
𝜕𝑥
∂ẋ
∂x
−   𝐶1𝜌𝑎Δ𝑥
+ 𝐶1𝜌𝑎Δ𝑥
𝜕𝑥̇
𝜕𝑥
𝜕𝑥̇
𝜕𝑥
if  
if
𝜕𝑥̇
𝜕𝑥
𝜕𝑥̇
𝜕𝑥
< 0
≥ 0,
(24.9)
where 𝐶1  is  a  dimensionless  constant  and  𝑎  is  the  local  sound  speed.    The  linear  term 
rapidly  damps  numerical  oscillations  behind  the  shock  front  (Figure  24.3).    A  similar 
form was proposed independently by Noh about the same time.
LS-DYNA Theory Manual 
Artificial Bulk Viscosity 
In  an  interesting  aside,  Wilkins  [1980]  discusses  work  by  Kuropatenko  who, 
given  an  equation of  state,  derived  a  q  by solving  the  jump  conditions  for  pressure  in 
terms of a change in the particle velocity, Δ𝑢.  For an equation of state of the form, 
𝑝 = 𝐾 (−
𝜌0
− 1),
pressure across the shock front is given by [Wilkins 1980] 
𝑝 = 𝑝0 + 𝜌0
(Δ𝑢)2
+ 𝜌0|Δ𝑢| [
2⁄
+ 𝑎 2]
,
(Δ𝑢)2
where 𝑎 is a sound speed 
𝑎 = (
2⁄
.
𝜌0
)
For a strong shock, Δ𝑢2 >> 𝑎2, we obtain the quadratic form 
and for a weak shock, Δ𝑢2 << 𝑎2, the linear form 
𝑞 = 𝜌0Δ𝑢2,
𝑞 = 𝜌0𝑎Δ𝑢,
(24.10)
(24.11)
(24.12)
(24.13)
(24.14)
Thus linear and quadratic forms for 𝑞 can be naturally derived.  According to Wilkins, 
the particular expressions for 𝑞 obtained by Kuropatenko offer no particular advantage 
over the expressions currently used in most computer programs. 
In  extending  the  one-dimensional  viscosity  formulations  to  multi-dimensions, 
most code developers have simply replaced the divergence of the velocity with, 𝜀̇𝑘𝑘, the 
trace of the strain rate tensor, and the  characteristic length with the square root of the 
area  A,  in  two  dimensions  and  the  cubic  root  of  the  volume  v  in  three  dimensions.  
These changes also give the default viscosities in the LS-DYNA codes: 
𝑞 = 𝜌 𝑙(𝐶0𝑙𝜀̇𝑘𝑘
𝑞 = 0
2 − 𝐶𝑙𝑎𝜀̇𝑘𝑘)
if 𝜀̇𝑘𝑘 < 0
if 𝜀̇𝑘𝑘 ≥ 0
(24.15)
where  𝐶0  and  𝐶1  are  dimensionless  constants  which  default  to  1.5  and  0.06, 
respectively, where 1 = √𝐴 in 2D, and √𝑣3
 in 3D, a is the local sound speed, 𝐶0 defaults 
to 1.5 and 𝐶1 defaults to 0.06. 
In  converging  two-  and  three-dimensional  geometries,  the  strain  rate  𝜀̇𝑘𝑘  is 
negative and the 𝑞 term in Equation (24.15) is nonzero, even though no shocks may be 
generated.    This  results  in  nonphysical  𝑞  heating.    When  the  aspect  ratios  of  the 
elements are poor (far from unity), the use of a characteristic length based on √𝐴 or √𝑣3
can  also  result  in  nonphysical  𝑞  heating  and  even  occasional  numerical  instabilities.  
Wilkins  uses  a  bulk  viscosity  that  is  based  in  part  on  earlier  work  by  Richards  [1965]
Artificial Bulk Viscosity 
LS-DYNA Theory Manual 
that extends the von Neumann and Richtmyer formulations in a way that avoids these 
problems.  This latter 𝑞 may be added in the future if the need arises. 
Wilkins’ 𝑞 is defined as: 
𝑞 = 𝐶0𝜌𝑙2 (
)
𝑑𝑠
𝑑𝑡
− 𝐶𝑙𝜌𝑙𝑎∗ 𝑑𝑠
𝑑𝑡
𝑞 = 0
 if  𝜀̇𝑘𝑘 < 0
if
𝑑𝑠
𝑑𝑡
≥ 0
(24.16)
where 𝑙 and 𝑑𝑠
𝑑𝑡 are the thickness of the element and the strain rate in the direction of the 
acceleration,  respectively,  and  𝑎∗  is  the  sound  speed  defined  by  (p/𝜌)1/2  if  𝑝 > 0.    We 
use the local sound speed in place of 𝑎∗ to reduce the noise at the low stress levels that 
are typical of our applications. 
Two disadvantages are associated with Equation (24.16).  To compute the length 
parameter and the strain rate, we need to know the direction of the acceleration through 
the element.  Since the nodal force vector becomes the acceleration vector in the explicit 
integration  scheme,  we  have  to  provide  extra  storage  to  save  the  direction.    In  three 
dimensions our present storage capacity is marginal at best and sacrificing this storage 
for storing the direction would make it even more so.  Secondly, we need to compute l 
and  𝑑𝑠
𝑑𝑡 which results in a noticeable increase in computer cost even in two dimensions.  
For most problems the additional refinement of Wilkins is not needed.  However, users 
must be aware of the pitfalls of Equation (24.15), i.e., when the element aspect ratios are 
poor or the deformations are large, an anomalous 𝑞 may be generated.
LS-DYNA Theory Manual 
Time Step Control 
25    
Time Step Control 
During the solution we loop through the elements to update the stresses and the 
right  hand  side  force  vector.    We  also  determine  a  new  time  step  size  by  taking  the 
minimum value over all elements. 
Δ𝑡𝑛+1 = 𝑎 ⋅ min{Δ𝑡1, Δ𝑡2, Δ𝑡3, . . . , Δ𝑡𝑁},
(25.1)
where 𝑁 is the number of elements.  For stability reasons the scale factor 𝑎 is typically 
set to a value of .90 (default) or some smaller value. 
25.1  Time Step Calculations for Solid Elements 
A critical time step size, Δ𝑡𝑒, is computed for solid elements from  
Δ𝑡𝑒 =
𝐿𝑒
{[𝑄 + (𝑄2 + 𝑐2)1/2]}
where 𝑄 is a function of the bulk viscosity coefficients 𝐶0 and 𝐶1: 
𝑄 = {
𝐶1𝑐 + 𝐶0𝐿𝑒|𝜀̇𝑘𝑘|
for 𝜀̇𝑘𝑘 ≤ 0
for 𝜀̇𝑘𝑘 > 0
(25.2)
(25.3)
𝐿𝑒 is a characteristic length: 
8 node solids:  
𝐿𝑒 =
4 node tetrahedras:  𝐿𝑒 = minimum altitude 
𝜐𝑒
𝐴𝑒max
𝜐𝑒  is  the  element  volume,  𝐴𝑒max  is  the  area  of  the  largest  side,  and  𝑐  is  the  adiabatic 
sound speed:   
𝑐 = [
4𝐺
3𝜌0
+
∂𝑝
∂𝜌
)
2⁄
]
,
(25.4)
where 𝜌 is the specific mass density.  Noting that:
Time Step Control 
LS-DYNA Theory Manual 
∂𝑝
∂𝜌
)
=
∂𝑝
∂𝜌
)
+
∂𝑝
∂𝑈
)
∂𝑈
∂𝜌
,
)
(25.5)
and  that  along  an  isentrope  the  incremental  energy,  𝑈,  in  the  units  of  pressure  is  the 
product of pressure, 𝑝, and the incremental relative volume, 𝑑𝑉: 
we obtain 
𝑑𝑈 = −𝑝𝑑𝑉,
𝑐 =
⎡ 4𝐺
⎢
3𝜌0
⎣
+
∂𝑝
∂𝜌
)
+
𝑝𝑉2
𝜌0
∂𝑝
∂𝑈
)
2⁄
⎤
⎥
𝜌⎦
.
(25.6)
(25.7)
For elastic materials with a constant bulk modulus the sound speed is given by: 
𝑐 = √
𝐸(1 − 𝜐)
(1 + 𝜐)(1 − 2𝜐)𝜌
(25.8)
where 𝐸 is Young’s modulus, and 𝜐 is Poisson’s ratio.  
25.2  Time Step Calculations for Beam and Truss Elements 
For the Hughes-Liu beam and truss elements, the time step size is given by: 
where 𝐿 is the length of the element and c is the wave speed: 
Δ𝑡𝑒 =
𝑐 = √
.
(25.9)
(25.10)
For  the  Belytschko  beam  the  time  step  size  given  by  the  longitudinal  sound 
speed  is  used  (Equation  (25.9)),  unless  the  bending-related  time  step  size  given  by 
[Belytschko and Tsay 1982] 
Δ𝑡𝑒 =  
𝑐√3𝐼 [
0.5𝐿
12𝐼 + 𝐴𝐿2 + 1
𝐴𝐿2]
(25.11)
is smaller, where 𝐼 and 𝐴 are the maximum value of the moment of inertia and area of 
the cross section, respectively. 
Comparison  of  critical  time  steps  of  the  truss  versus  the  elastic  solid  element 
shows  that  it  if  Poisson's  ratio,  𝜐,  is  nonzero  the  solid  elements  give  a  considerably 
smaller stable time step size.  If we define the ratio, 𝛼, as:
LS-DYNA Theory Manual 
Time Step Control 
𝛼 =
Δ𝑡continuum
Δ𝑡rod
=
𝐶rod
𝐶continuum
= √
(1 + 𝜐)(1 − 2𝜐)
,
1 − 𝜐
(25.12)
we obtain the results in Table 22.1 where we can see that as υ approaches .5 𝛼 → 0. 
0 
1. 
0.2 
0.949 
0.3 
0.862 
0.4 
0.683 
0.45 
0.513 
0.49 
0.242 
0.50 
0.0 
Table 22.1.  Comparison of critical time step sizes for a truss versus a solid element. 
25.3  Time Step Calculations for Shell Elements 
For the shell elements, the time step size is given by: 
where 𝐿𝑠 is the characteristic length and 𝑐 is the sound speed:   
Δ𝑡𝑒 =
𝐿𝑠
𝑐 = √
𝜌(1 − 𝜈2)
.
(25.13)
(25.14)
Three user options exists for choosing the characteristic length.  In the default or 
first option the characteristic length is given by: 
𝐿𝑠 =
(1 + 𝛽)𝐴𝑠
max(𝐿1, 𝐿2, 𝐿3, (1 − 𝛽)𝐿4)
(25.15)
where  𝛽 = 0  for  quadrilateral  and  1  for  triangular  shell  elements,  𝐴𝑠  is  the  area,  and 
𝐿𝑖, (𝑖 = 1. . . .4)  is  the  length  of  the  sides  defining  the  shell  elements.    In  the  second 
option a more conservative value of 𝐿𝑠 is used: 
(1 + 𝛽)𝐴𝑠
,
max(𝐷1, 𝐷2)
𝐿𝑠 =
(25.16)
where 𝐷𝑖(𝑖 = 1,2) is the length of the diagonals.  The third option provides the largest 
time  step  size  and  is  frequently  used  when  triangular  shell  elements  have  very  short 
altitudes.  The bar wave speed, Equation (21.10), is used to compute the time step size 
and 𝐿𝑠 is given by 
𝐿𝑠 = max [
(1 + 𝛽)𝐴𝑠
max(𝐿1, 𝐿2, 𝐿3, (1 − 𝛽)𝐿4)
, min(𝐿1, 𝐿2, 𝐿3, 𝐿4 + 𝛽1020)]. 
(25.17)
A  comparison  of  critical  time  steps  of  truss  versus  shells  is  given  in  Table  22.2 
with 𝛽 defined as:
Time Step Control 
LS-DYNA Theory Manual 
𝛽 =
Δ𝑡2D-continuum
Δ𝑡rod
=
𝐶rod
= √1 − 𝜐2.
(25.18)
0 
1.0 
0.2 
0.98 
0.3 
0.954 
0.4 
0.917 
0.5 
0.866 
Table 22.2.  Comparison of critical time step sizes for a truss versus a shell element. 
25.4  Time Step Calculations for Solid Shell Elements 
A critical time step size, Δ𝑡𝑒 is computed for solid shell elements from  
𝜐𝑒
𝑐𝐴𝑒max
where 𝜐𝑒 is the element volume, 𝐴𝑒max is the area of the largest side, and 𝑐 is the plane 
stress sound speed given in Equation (25.14). 
Δ𝑡𝑒 =
(25.19)
,
25.5  Time Step Calculations for Discrete Elements 
For  spring  elements  such  as  that  in  Figure  25.1  there  is  no  wave  propagation 
speed 𝑐 to calculate the critical time step size. 
The  eigenvalue  problem  for  the  free  vibration  of  spring  with  nodal  masses  𝑚1 
and 𝑚2, and stiffness, 𝑘, is given by: 
[ 𝑘 −𝑘
−𝑘
] [
𝑢1
𝑢2
] − 𝜔2 [
𝑚1
𝑚2
] [
𝑢1
𝑢2
] = [0
].
(25.20)
Since  the  determinant  of  the  characteristic  equation  must  equal  zero,  we  can  solve  for 
the maximum eigenvalue: 
det [
𝑘 − 𝜔2𝑚1
−𝑘
−𝑘
𝑘 − 𝜔2𝑚2
] = 0 → 𝜔max
2 =
𝑘(𝑚1 + 𝑚2)
𝑚1 ⋅ 𝑚2
, 
(25.21)
LS-DYNA Theory Manual 
Time Step Control 
m1 = 0.5M1 ;
M1 = 
nodal mass
m2 = 0.5M2 ;
M2 = 
nodal mass
Figure 25.1.  Lumped spring mass system. 
Recalling the critical time step of a truss element: 
        Δ𝑡 ≤
𝜔max =
⎫
}}
⎬
2𝑐
}}
ℓ ⎭
    Δ𝑡 ≤
𝜔max
, 
(25.22)
and approximating the spring masses by using 1/2 the actual nodal mass, we obtain: 
    Δ𝑡 = 2√
𝑚1𝑚2
𝑚1 + 𝑚2
.
(25.23)
Therefore, in terms of the nodal mass we can write the critical time step size as: 
Δ𝑡𝑒 = √
2𝑀1𝑀2
𝑘(𝑀1 + 𝑀2)
.
(25.24)
The springs used in the contact interface are not checked for stability.
LS-DYNA Theory Manual 
Boundary and Loading Conditions 
26    
Boundary and Loading Conditions 
26.1  Pressure Boundary Conditions 
Consider pressure loadings on boundary ∂b1 in Equation (2.4).  To carry out the 
surface integration indicated by the integral 
a  Gaussian  quadrature  rule  is  used.    To  locate  any  point  of  the  surface  under 
consideration, a position vector, 𝑟, is defined: 
∫ 𝑁𝑡𝑡𝑑𝑠
∂𝑏1
,
(26.1)
where 
𝑟 = 𝑓1(𝜉 , 𝜂)𝑖1 + 𝑓2((𝜉 , 𝜂)𝑖2 + 𝑓3(𝜉 , 𝜂)𝑖3,
𝑓𝑖(𝜉 , 𝜂) = ∑ 𝜙𝑗𝑥𝑖
,
𝑗=1
(26.2)
(26.3)
and 𝑖1, 𝑖2, 𝑖3 are unit vectors in the 𝑥1, 𝑥2, 𝑥3directions . 
Nodal  quantities  are  interpolated  over  the  four-node  linear  surface  by  the 
functions 
𝜙𝑖 =
(1 + 𝜉 𝜉𝑖)(1 + 𝜂𝜂𝑖),
(26.4)
so  that  the  differential  surface  area  𝑑𝑠  may  be  written  in  terms  of  the  curvilinear 
coordinates as 
where |𝐽| is the surface Jacobian defined by 
𝑑𝑠 = |𝐽|𝑑𝜉𝑑𝜂,
|𝐽| = ∣
∂𝑟
∂𝜉
×
∂𝑟
∂𝜂
2⁄
∣ = (𝐸𝐺 − 𝐹2)
,
(26.5)
(26.6)
in which
Boundary and Loading Conditions 
LS-DYNA Theory Manual 
x3
i3
i2
r(ξ,η)
x1
x2
i1
Figure 26.1.  Parametric representation of a surface segment. 
𝐸 =
𝐹 =
𝐺 =
∂𝑟
∂𝜉
∂𝑟
∂𝜉
∂𝑟
∂𝜂
⋅
⋅
⋅
∂𝑟
∂𝜉
∂𝑟
∂𝜂
∂𝑟
∂𝜂
, 
, 
. 
A unit normal vector 𝐧 to the surface segment is given by 
𝐧 = |𝐽| −1 (
∂𝐫
∂𝜉
×
∂𝐫
∂𝜂
),
and the global components of the traction vector can now be written 
𝑡𝑖 = 𝑛𝑖 ∑ 𝜙𝑗𝑝𝑗
𝑗=1
,
where 𝑝𝑗 is the applied pressure at the jth node. 
The surface integral for a segment is evaluated as: 
(26.7)
(26.8)
(26.9)
∫ ∫ 𝑁𝑡𝑡|𝐽|𝑑𝜉 𝑑𝜂
−1
−1
.
(26.10)
One  such  integral  is  computed  for  each  surface  segment  on  which  a  pressure  loading 
acts.    Note  that  the  Jacobians  cancel  when  Equations  (26.8)  and  (26.7)  are  put  into 
Equation (26.10).  Equation (26.10) is evaluated with one-point integration analogous to 
that employed in the volume integrals.  The area of an element side is approximated by 
4|𝐽| where  |𝐽| = |𝐽(0, 0)|.
LS-DYNA Theory Manual 
Boundary and Loading Conditions 
26.2  Transmitting Boundaries 
Transmitting  boundaries  are  available  only  for  problems  that  require  the 
modeling of semi-infinite or infinite domains with solid elements and therefore are not 
available for beam or shell elements.  Applications of this capability include problems in 
geomechanics and underwater structures.   
The  transmitting  or  silent  boundary  is  defined  by  providing  a  complete  list  of 
boundary  segments.    In  the  approach  used,  discussed  by  Cohen  and  Jennings  [1983] 
who in turn credit the method to Lysmer and Kuhlemeyer [1969], viscous normal shear 
stresses in Equation (23.11) are applied to the boundary segments: 
𝛔normal = −𝜌𝑐𝑑𝐕normal
𝛔shear = −𝜌𝑐𝑠𝐕tan,
(26.11)
(26.12)
where 𝜌, 𝑐𝑑,and 𝑐𝑠 are the material density, dilatational wave speed, and the shear wave 
speed  of  the  transmitting  media  respectively.    The  magnitude  of  these  stresses  is 
proportional  to  the  particle  velocities  in  the  normal,  𝐕normal,  and  tangential,  𝐕tan, 
directions.  The material associated with each transmitting segment is identified during 
initialization  so  that  unique  values  of  the  constants  𝜌, 𝑐𝑑,  and  𝑐𝑠  can  be  defined 
automatically. 
26.3  Kinematic Boundary Conditions 
In  this  subsection,  the  kinematic  constraints  are  briefly  reviewed.    LS-DYNA 
tracks  reaction  forces  for  each  type  of  kinematic  constraint  and  provides  this 
information as output if requested.  For the prescribed boundary conditions, the input 
energy is integrated and included in the external work. 
26.4  Displacement Constraints 
Translational and rotational boundary constraints are imposed either globally or 
locally by setting the constrained acceleration components to zero.  If nodal single point 
constraints  are  employed,  the  constraints  are  imposed  in  a  local  system.    The  user 
defines the local system by specifying a vector 𝐮1 in the direction of the local x-axis 𝐱l, 
and a local in-plane vector 𝐯l.  After normalizing 𝐮1, the local 𝐱𝑙, 𝐲𝑙and 𝐳l axes are given 
by:
Boundary and Loading Conditions 
LS-DYNA Theory Manual 
𝐱𝑙 =
𝐮𝑙
‖𝐮𝑙‖
𝐳𝑙 =
𝐱𝑙 × 𝐯𝑙
‖𝐱𝑙 × 𝐯𝑙‖
𝐲𝑙 = 𝐳𝑙 × 𝐱𝑙.
(26.13)
(26.14)
(26.15)
A  transformation  matrix  𝐪  is  constructed  to  transform  the  acceleration 
components to the local system: 
𝐪 =
𝐱𝑙
⎤
⎡
⎥⎥
⎢⎢
, 
𝐲𝑙
T ⎦
𝐳𝑙
⎣
(26.16)
and the nodal translational and rotational acceleration vectors 𝐚𝐼 and 𝛚̇ 𝐼, for node I are 
transformed to the local system:  
𝐚𝐼1 = 𝐪𝐚𝐼
𝛚̇ 𝐼𝑙
= 𝐪𝛚̇ 𝐼,
(26.17)
(26.18)
and  the  constrained  components  are  zeroed. 
transformed back to the global system: 
  The  modified  vectors  are  then 
𝐚𝐼 = 𝐪T𝐚𝐼1
𝛚̇ 𝐼 = 𝐪T𝛚̇ 𝐼𝑙
(26.19)
(26.20)
26.5  Prescribed Displacements, Velocities, and 
Accelerations 
Prescribed  displacements,  velocities,  and  accelerations  are  treated  in  a  nearly 
identical  way  to  displacement  constraints.    After  imposing  the  zero  displacement 
constraints,  the  prescribed  values  are  imposed  as  velocities  at  time,  𝑡𝑛+1/2.    The 
acceleration  versus  time  curve  is  integrated  or  the  displacement  versus  time  curve  is 
differentiated  to  generate  the  velocity  versus  time  curve.    The  prescribed  nodal 
components are then set.
LS-DYNA Theory Manual 
Boundary and Loading Conditions 
26.6  Body Force Loads 
Body  force  loads  are  used  in  many  applications.    For  example,  in  structural 
analysis the base accelerations can be applied in the simulation of earthquake loadings, 
the  gun  firing  of  projectiles,  and  gravitational  loads.    The  latter  is  often  used  with 
dynamic relaxation to initialize the internal forces before proceeding with the transient 
response  calculation.    In  aircraft  engine  design  the  body  forces  are  generated  by  the 
application of an angular velocity of the spinning structure.  The generalized body force 
loads are available if only part of the structure is subjected to such loadings, e.g., a bird 
striking a spinning fan blade. 
For base accelerations and gravity we can fix the base and apply the loading as 
part of the body force loads element by element according to Equation (22.18) 
𝐟𝑒body = ∫ 𝜌𝐍T𝐍𝐚base𝑑𝜐
  𝜐𝑚
= 𝐦𝑒𝐚base,
(26.21)
where 𝐚base is the base acceleration and 𝐦𝑒 is the element (lumped) mass matrix.
LS-DYNA Theory Manual 
Time Integration 
27    
Time Integration 
27.1  Background 
Consider the single degree of freedom damped system in Figure 27.1. 
p(t)
u(t)
 - displacements
Figure 27.1.  Single degree of freedom damped system. 
Forces acting on mass m are shown in Figure 27.2. 
The equations of equilibrium are obtained from d'Alembert’s principle 
𝑓𝐼 + 𝑓𝐷 + 𝑓int = 𝑝(𝑡)
(27.1)
fI
inertia force
p(t) external forces
elastic force
fs
fD
damping forces
Figure 27.2.  Forces acting on mass, m
Time Integration 
LS-DYNA Theory Manual 
𝑓𝐼 = 𝑚𝑢̈;    𝑢̈ =
𝑓𝐷 = 𝑐𝑢̇;    𝑢̇ =
𝑓int = 𝑘 ⋅ 𝑢;
𝑑2𝑢
𝑑𝑡2   acceleration 
𝑑𝑢
 velocity 
𝑑𝑡
𝑢 displacement
(27.2)
where 𝑐 is the damping coefficient, and k is the linear stiffness.  For critical damping 𝑐 =
ccr.    The  equations  of  motion  for  linear  behavior  lead  to  a  linear  ordinary  differential 
equation, o.d.e.: 
𝑚𝑢̈ + 𝑐𝑢̇ + 𝑘𝑢 = 𝑝(𝑡)
(27.3)
but  for  the  nonlinear  case  the  internal  force  varies  as  a  nonlinear  function  of  the 
displacement, leading to a nonlinear o.d.e.: 
𝑚𝑢̈ + 𝑐𝑢̇ + 𝑓int(𝑢) = 𝑝(𝑡)
(27.4)
Analytical  solutions  of  linear  ordinary  differential  equations  are  available,  so 
instead  we  consider  the  dynamic  response  of  linear  system  subjected  to  a  harmonic 
loading.  It is convenient to define some commonly used terms: 
Harmonic loading:  𝑝(𝑡) = 𝑝0sin𝜛𝑡 
Circular frequency:  𝜔 = √ 𝑘
2𝜋 = 1
Natural frequency:  𝑓 = 𝜔
= 𝑐
𝜉 = 𝑐
Damping ratio: 
𝑐𝑐𝑟
𝑇     𝑇 = period 
2𝑚𝜔 
𝑚 for single degree of freedom 
Damped vibration frequency: 
Applied load frequency:  𝛽 = 𝜔̅̅̅̅̅
𝜔 
 𝜔0 = 𝜔√1 − 𝜉 2 
The closed form solution is: 
𝑢̇0
𝑝0
sin𝜔𝑡 +
𝑢(𝑡) = 𝑢0cos𝜔𝑡 +
1 − 𝛽2 (sin𝜔̅̅̅̅𝑡 − 𝛽sin𝜔𝑡)
homogeneous solution               steady state       transient
particular solution
(27.5)
with the initial conditions: 
𝑢0 = initial displacement 
𝑢̇0 = initial velocity 
𝑝0
= static displacement 
For  nonlinear  problems,  only  numerical  solutions  are  possible.    LS-DYNA  uses 
the explicit central difference scheme to integrate the equations of motion.
LS-DYNA Theory Manual 
Time Integration 
27.2  The Central Difference Method 
The semi-discrete equations of motion at time n are: 
(27.6)
where 𝐌 is the diagonal mass matrix, 𝐏𝑛 accounts for external and body force loads, 𝑭 𝑛 
is the stress divergence vector, and 𝐇𝑛 is the hourglass resistance.  To advance to time 
𝑡𝑛+1, we use central difference time integration: 
𝐌𝐚𝑛 = 𝐏𝑛 − 𝐅𝑛 + 𝐇𝑛,
𝐚𝑛 = 𝐌−1(𝐏𝑛 − 𝐅𝑛 + 𝐇𝑛),
𝐯𝑛+1
2⁄ = 𝐯𝑛−1
2⁄ + 𝐚𝑛Δ𝑡𝑛,
𝐮𝑛+1 = 𝐮𝑛 + 𝐯𝑛+1
2⁄ Δ𝑡𝑛+1
2⁄ ,
(27.7)
(27.8)
(27.9)
where 
(Δ𝑡𝑛 + Δ𝑡𝑛+1)
,
and  𝐯 and  𝐮 are the global nodal velocity and  displacement vectors, respectively.  We 
update the geometry by adding the displacement increments to the initial geometry:  
Δ𝑡𝑛+1
2⁄ =
(27.10)
𝐱𝑛+1 = 𝐱0 + 𝐮𝑛+1.
(27.11)
We have found that, although more storage is required to store the displacement vector 
the results are much less sensitive to round-off error. 
27.3  Stability of Central Difference Method 
The  stability  of  the  central  difference  scheme  is  determined  by  looking  at  the 
stability of a linear system.  The system of linear equations in uncoupled into the modal 
equations  where  the  modal  matrix  of  eigenvectors,  𝛟,  are  normalized  with  respect  to 
the mass and linear stiffness matrices 𝐊, and 𝐌, respectively, such that: 
𝛟T𝐌𝛟 = I
𝛟T𝐊𝛟 = ω2.
(27.12)
With this normalization, we obtain for viscous proportional damping the decoupling of 
the damping matrix, 𝐂: 
The equations of motion in the modal coordinates 𝐱 are: 
𝛟T𝐂𝛟 = 2𝜉𝜔
𝑥̈ + 2𝜉ω𝑥̇ + ω2𝑥 = 𝛟𝐓𝐩⏟
.
=Y
(27.13)
(27.14)
With central differences we obtain for the velocity and acceleration:
Time Integration 
LS-DYNA Theory Manual 
𝑥̇𝑛 =
𝑥𝑛+1 − 𝑥𝑛−1
2Δ𝑡
𝑥̈𝑛 =
𝑥𝑛+1 − 2𝑥𝑛 + 𝑥𝑛−1
Δ𝑡2
.
Substituting 𝑥̇𝑛 and 𝑥̈𝑛 into equation of motion at time 𝑡𝑛 leads to: 
𝑥𝑛+1 =
2 − 𝜔2Δ𝑡2
1 + 2𝜉𝜔Δ𝑡2 𝑥𝑛 −
1 − 2𝜉𝜔Δ𝑡
1 + 2𝜉𝜔Δ𝑡
𝑥𝑛−1 +
Δ𝑡2
1 + 2𝜉𝜔Δ𝑡2 𝑌𝑛, 
which in matrix form leads to 
𝑥𝑛 = 𝑥𝑛,
[
𝑥𝑛+1
𝑥𝑛
] =
2 − 𝜔2Δ𝑡2
1 + 2𝜉𝜔Δ𝑡
⎡
⎢
⎣
−
1 − 2𝜉𝜔Δ𝑡
1 + 2𝜉𝜔Δ𝑡
⎤
⎥
⎦
[
𝑥𝑛
𝑥𝑛−1
] +
Δ𝑡2
⎡
⎢
1 + 2𝜉𝜔Δ𝑡2
⎣
⎤
⎥
⎦
𝑌𝑛, 
or 
𝐱̂𝑛+1 = 𝐀𝐱̂𝑛 + 𝐋𝐘𝑛,
(27.15)
(27.16)
(27.17)
(27.18)
(27.19)
(27.20)
where, 𝐀 is the time integration operator for discrete equations of motion.  After 𝑚 time 
steps with 𝐋 = 0 we obtain: 
As 𝑚 approaches infinity, 𝐀 must remain bounded.   
𝐱̂𝑚 = 𝐀𝑚𝐱̂0.
A spectral decomposition of 𝐴 gives: 
𝐀𝑚 = (𝐏T𝐉𝐏)
= 𝐏T𝐉𝑚𝐏,
(27.21)
(27.22)
where, 𝐏, is the orthonormal matrix containing the eigenvectors of 𝐀, and 𝐉 is the Jordan 
form  with  the  eigenvalues  on  the  diagonal.    The  spectral  radius,  𝜌(𝐀),  is  the  largest 
eigenvalue of 𝐀 = max [diag.  (J)].  We know that 𝐉𝑚, is bounded if and only if: 
∣𝜌(𝐀)∣ ≤ 1.
Consider the eigenvalues of 𝐴 for the undamped equation of motion 
Det [∣2 − 𝜔2Δ𝑡2 −1
∣ − 𝜆∣1 −1
∣] = 0,
−(2 − 𝜔2Δ𝑡2 − 𝜆) ⋅ 𝜆 + 1 = 0,
𝜆 =
2 − 𝜔2Δ𝑡2
± √
(2 − 𝜔2Δ𝑡2)2
− 1.
(27.23)
(27.24)
(27.25)
(27.26)
The requirement that |𝜆| ≤ 1 leads to:
LS-DYNA Theory Manual 
Time Integration 
Δ𝑡 ≤
𝜔max
,
as the critical time step.  For the damped equations of motion we obtain: 
Δ𝑡 ≤
𝜔max
(√1 + 𝜉 2 − 𝜉 ).
(27.27)
(27.28)
Thus, damping reduces the critical time step size.  The time step size is bounded 
by  the  largest  natural  frequency  of  the  structure  which,  in  turn,  is  bounded  by  the 
highest frequency of any individual element in the finite element mesh. 
27.4  Subcycling (Mixed Time Integration) 
The time step size, Δ𝑡, is always limited by a single element in the finite element 
mesh.    The  idea  behind  subcycling  is  to  sort  elements  based  on  their  step  size  into 
groups whose step size is some even multiple of the smallest element step size, 2(𝑛−1)Δ𝑡, 
for integer values of 𝑛 greater than or equal to 1.  For example, in Figure 27.3 the mesh 
on the right because of the thin row of elements is three times more expensive than the 
mesh on the left 
The  subcycling  in  LS-DYNA  is  based  on  the  linear  nodal  interpoation  partition 
subcycling algorithm of Belytschko, Yen, and Mullen [1979], and Belytschko [1980].  In 
their implementation the steps are: 
1. 
2. 
3. 
Assign each node, 𝑖, a time step size, Δ𝑡𝑗, according to: 
Δ𝑡𝑖 = min (2
𝜔𝑗⁄ ) over all elements 𝑗, connected to node 𝑖 
Assign each element, 𝑗, a time step size, Δ𝑡𝑗, according to: 
Δ𝑡𝑗   = min(Δ𝑡𝑖) over all nodes, 𝑖, of element, 𝑗 
Group elements into blocks by time step size for vectorization. 
Figure  27.3.    The  right  hand  mesh  is  much  more  expensive  to  compute  than 
the left hand due to the presence of the thinner elements.
Time Integration 
LS-DYNA Theory Manual 
In LS-DYNA we desire to use constant length vectors as much as possible even if 
it means updating the large elements incrementally with the small time step size.  We 
have found that doing this decreases costs and stability is unaffected. 
Hulbert  and  Hughes  [1988]  reviewed  seven subcycling  algorithms  in  which  the 
partitioning  as  either  node  or  element  based.    The  major  differences  within  the  two 
subcycling  methods  lie  in  how  elements  along  the  interface  between  large  and  small 
elements  are  handled,  a  subject  which  is  beyond  the  scope  of  this  theoretical  manual.  
Nevertheless,  they  concluded  that  three  of  the  methods  including  the  linear  nodal 
interpolation method chosen for LS-DYNA, provide both stable and accurate solutions 
for  the  problems  they  studied.    However,  there  was  some  concern  about  the  lack  of 
stability  and  accuracy  proofs  for  any  of  these  methods  when  applied  to  problems  in 
structural mechanics. 
The  implementation  of  subcycling  currently  includes  the  following  element 
classes and contact options: 
• 
• 
• 
• 
• 
Solid elements 
Beam elements 
Shell elements 
Brick shell elements 
Penalty based contact algorithms. 
but  intentionally  excludes  discrete  elements  since  these  elements  generally  contribute 
insignificantly  to  the  calculational  costs.    The  interface  stiffnesses  used  in  the  contact 
algorithms  are  based  on  the  minimum  value  of  the  slave  node  or  master  segment 
stiffness and, consequently, the time step size determination for elements on either side 
of the interface is assumed to be decoupled; thus, scaling penalty values to larger values 
when subcycling is active can be a dangerous exercise indeed.  Nodes that are included 
in constraint equations, rigid bodies, or in contact with rigid walls are always assigned 
the smallest time step sizes. 
To  explain  the  implementation  and  the  functioning  of  subcycling,  we  consider 
the beam shown in Figure 27.4 where the beam elements on the right (material group 2) 
have  a  Courant  time  step  size  exactly  two  times  greater  than  the  elements  on  the  left.  
The  nodes  attached  to  material  group  2  will  be  called  minor  cycle  nodes  and  the  rest, 
major  cycle  nodes.    At  time  step  𝑛 = 𝑚𝑘  all  nodal  displacements  and  element  stresses 
are known, where 𝑚 is the ratio between the largest and smallest time step size, 𝑘 is the 
number of major time steps, and 𝑛 is the number of minor time steps.  In Figures 27.5 
and 27.6, the update of the state variables to the next major time step 𝑘 + 1 is depicted.  
The stress state in the element on the material interface in group 1 is updated during the 
minor  cycle  as  the  displacement  of  the  major  cycle  node  shared  by  this  element  is 
assumed  to  vary  linearly  during  the  minor  cycle  update.    This  linear  variation  of  the 
major  cycle  nodal  displacements  during  the  update  of  the  element  stresses  improves 
accuracy and stability.
LS-DYNA Theory Manual 
Time Integration 
Material Group 1
Material Group 2
E2 = 4E1
A2 = A1
2 = ρ
1 
F(t)
Figure 27.4.  Subcycled beam problem from Hulbert and Hughes [1988]. 
In  the  timing  study  results  in  Table  24.1,  fifty  solid  elements  were  included  in 
each  group  for  the  beam  depicted  in  Figure  27.4,  and  the  ratio  between  𝐸2  to  𝐸1  was 
varied from 1 to 128 giving a major time step size greater than 10 times the minor.  Note 
that  as  the  ratio  between  the  major  and  minor  time  step  sizes  approaches  infinity  the 
reduction  in  cost  should  approach  50  percent  for  the  subcycled  case,  and  we  see  that 
this is indeed the case.  The effect of subcycling for the more expensive fully integrated 
elements is greater as may be expected.  The overhead of subcycling for the case where 
𝐸1 = 𝐸2 is relatively large.  This provides some insight into why a decrease in speed is 
often observed when subcycling is active.  For subcycling to have a significant effect, the 
ratio of the major to minor time step size should be large and the number of elements 
having the minor step size should be small.  In crashworthiness applications the typical 
mesh is very well planned and generated to have uniform time step sizes; consequently, 
subcycling will probably give a net increase in costs.
Time Integration 
LS-DYNA Theory Manual 
u2
v2
u2
v2
Solve for accelerations, velocities, and displacements
Solve for minor cycle stresses
u1
v1
u1
v1
Figure 27.5.  Timing diagram for subcycling algorithm based on  linear nodal
interpolations. 
Case  1  one  point 
integration  with 
elastic  material 
model 
Number of cycles 
cpu time(secs) 
𝐸2 = 𝐸1 
𝐸2 = 4𝐸1 
𝐸2 = 16𝐸1 
𝐸2 = 64𝐸1 
𝐸2 = 128𝐸1 
178 
178 
367 
367 
714 
715 
1417 
1419 
2003 
2004 
4.65 
5.36 (+15.%) 
7.57 
7.13 (-6.0%) 
12.17 
10.18 (-20.%) 
23.24 
16.39 (-29.%) 
31.89 
22.37 (-30.%) 
Case  2  eight  point 
integration  with 
orthotropic 
material model 
Number of cycles 
cpu time(secs)
LS-DYNA Theory Manual 
Time Integration 
u2
v2
u2
v2
u1
v1
Solve for minor cycle accelerations, velocities, and displacements
u2
v2
u2
v2
u1
v1
Update stress for all elements
Figure 27.6.  Timing diagram for subcycling algorithm based on linear nodal
interpolations. 
𝐸2 = 𝐸1 
𝐸2 = 4𝐸1 
𝐸2 = 16𝐸1 
𝐸2 = 64𝐸1 
𝐸2 = 128𝐸1 
180 
180 
369 
369 
718 
719 
1424 
1424 
2034 
2028 
22.09 
22.75 (+3.0%) 
42.91 
34.20 (-20.%) 
81.49 
54.75 (-33.%) 
159.2 
97.04 (-39.%) 
226.8 
135.5 (-40.%) 
Table 24.1.  Timing study showing effects of the ratio of the major to minor time step 
size. 
The  impact  of  the  subcycling  implementation  in  the  software  has  a  very 
significant  effect  on  the  internal  structure.    The  elements  in  LS-DYNA  are  now  sorted 
three times
Time Integration 
LS-DYNA Theory Manual 
Time Integration Loop
update velocities
write databases
update displacements
and new geometry
kinematic based contact
and rigid walls
update accelerations and
apply kinematic b.c.'s
update current time and
check for termination
Start
apply force boundary
conditions
process penalty based
contact interfaces
process brick,beam, 
shell elements
process discrete
elements
Figure 27.7.  The time integration loop in LS-DYNA. 
By element number in ascending order. 
By material number for large vector blocks. 
• 
• 
By  connectivity  to  insure  disjointness  for  right  hand  side  vectorization  which  is 
• 
very important for efficiency. 
Sorting  by  Δ𝑡,  interact  with  the  second  and  third  sorts  and  can  result  in  the 
creation of much smaller vector blocks and result in higher cost per element time step.  
During the simulation elements can continuously change in time step size and resorting 
may  be  required  to  maintain  stability;  consequently,  we  must  check  for  this 
continuously.    Sorting  cost,  though  not  high  when  spread  over  the  entire  calculation, 
can become a factor that results in higher overall cost if done too frequently especially if 
the factor, m, is relatively small and the ratio of small to large elements is large.
LS-DYNA Theory Manual 
Rigid Body Dynamics 
28    
Rigid Body Dynamics 
A  detailed  discussion  of  the  rigid  body  algorithm  is  presented  by  Benson  and 
Hallquist [1986] and readers are referred to this publication for more information.  The 
equations of motion for a rigid body are given by 
𝑥,
𝑀𝜌𝒙̈ = 𝒇𝜌
𝑱𝜌𝝎̇ + 𝝎 × 𝑱𝜌𝝎 = 𝒇𝜌
𝜔,
(28.1)
(28.2)
where  𝑀𝜌  is  the  physical  mass,  𝑱𝜌  is  the  physical  inertia  tensor,  𝒙  is  the  location  of  the 
𝜔 are the forces and 
center of mass, 𝝎 is the angular velocity of the body, and 𝒇𝜌
torques  applied  to  the  rigid  body  through  *LOAD_RIGID_BODY.  These  are  equations 
that  can  be  found  in  a  standard  text  book  on  rigid  body  mechanics.    The  physical 
properties of a rigid body may come from three sources, these are 
𝑥 and 𝒇𝜌
1.Integration of the mass density 𝜌 over a region 𝑉 occupied by the rigid body, for 
which  𝑀𝜌 = ∫ 𝜌𝑑𝑉,  and    𝑱𝜌 = ∫ 𝜌(𝒚 − 𝒙)⨂(𝒚 − 𝒙)𝑑𝑉.  The  initial  rigid  body 
coordinate  𝒙  is  in  this  case  determined  from  𝒙 =
∫ 𝜌𝒚𝑑𝑉
𝑀𝜌
.  Here  𝒚  is  the  integrand 
variable. 
2.Specifying  properties  using  *PART_INERTIA,  for  which  𝑀𝜌,  𝑱𝜌  and  initial 
coordinate 𝒙 is simply specified in the keyword input deck. 
3.For  a  nodal  rigid  body,  *CONSTRAINED_NODAL_RIGID_BODY,  the  physical 
properties vanish, i.e., 𝑀𝜌 = 0 and 𝑱𝜌 = 𝟎, and the position is arbitrary. 
All  rigid  bodies  possess  slave  nodes,  which  play  a  role  when  rigid  bodies  in  LS-DYNA 
interact with their surroundings.  Slave nodes may come from the following. 
1.The  nodes  in  the  finite  element  mesh  for  the  part  specified  as  rigid  through 
*MAT_RIGID. 
2.Extra nodes definitions through *CONSTRAINED_EXTRA_NODES. 
3.The set used for a nodal rigid body in *CONSTRAINED_NODAL_RIGID_BODY.
Rigid Body Dynamics 
LS-DYNA Theory Manual 
We use 𝑆 to denote the set of slave nodes to the rigid body, and these are constrained to 
the rigid body through the equations 
𝒙𝑖 = 𝒙 + 𝑸(𝒙𝑖
0 − 𝒙0),
𝑸𝑖 = 𝑸,
(28.3)
(28.4)
for all 𝑖 ∈ 𝑆. Here we have introduced the orientations 𝑸 and 𝑸𝑖 of the rigid body and 
slave node 𝑖, respectively.  Furthermore, 𝒙𝑖 is the coordinate of slave node 𝑖 and we use 
superscript 0 to denote a quantity at time zero.  The time evolution of 𝑸 is 
𝑸̇ = 𝜴𝑸,
(28.5)
where  𝛀𝒓 = 𝝎 × 𝒓  for  an  arbitrary  vector  𝒓  and  𝑸 = 𝑰  (identity)  at  time  zero.    So 
equations (28.3) and (28.4) can equivalently be put in rate form 
𝒙̇𝑖 = 𝒙̇ + 𝝎 × 𝒓𝑖,
𝝎𝑖 = 𝝎,
(28.6)
(28.7)
where  𝒓𝑖 = 𝒙𝑖 − 𝒙  and  understandably  𝝎𝑖  rotational  velocity  of  slave  node  𝑖.  This  also 
determines  the  space  of  admissible  virtual  displacement  for  the  slave  nodes  in  the 
context  of  work  principles,  and  for  this  reason  we  use  a  compact  notation  for  this 
equation 
[
𝒙̇𝑖
𝝎𝑖
] = [
𝑰 −𝑹𝑖
] [ 𝒙̇
].
(28.8)
where 𝑹𝑖𝒓 = 𝒓𝑖 × 𝒓 for an arbitrary vector 𝒓. 
Slave nodes may have masses 𝑚𝑖, inertias 𝑱𝑖 and forces 𝒇𝑖
𝑥 and 𝒇𝑖
𝜔 associated with 
them.  The inertia properties may come from 
1.Mass contributions from deformable elements connected to the rigid body, either 
or 
through 
*CONSTRAINED_NODAL_RIGID_BODY or simply merged mesh. 
2.Lumped masses through *ELEMENT_MASS or *ELEMENT_INERTIA. 
*CONSTRAINED_EXTRA_NODES 
and the forces may come from 
1.External loads through *LOAD_NODE or *LOAD_SEGMENT. 
2.Contacts or fluid structure interaction (FSI) or similar. 
3.Internal forces on deformable nodes of a contiguous part. 
Note that these quantities exclude any contributions from and on the rigid body itself, 
𝜔. The motion of the slave nodes is governed 
as these are all collected in 𝑀𝜌, 𝑱𝜌, 𝒇𝜌
by their own equations of motion 
𝑥 and 𝒇𝜌
28-2 (Rigid Body Dynamics) 
𝑚𝑖𝒙̈𝑖 = 𝒇𝑖
𝑥,
LS-DYNA Theory Manual 
Rigid Body Dynamics 
𝑱𝑖𝝎̇𝑖 + 𝝎𝑖 × 𝑱𝑖𝝎𝑖 = 𝒇𝑖
𝜔,
(28.10)
for 𝑖 ∈ 𝑆. We seek a set of equations for the rigid body that combines (28.1)-(28.2) and 
(28.9)-(28.10)  by  condensing  out  the  dependence  of  the  slave  nodes  through  (28.6)-
(28.7). Differentiating (28.6)-(28.7) with respect to time yields 
𝒙̈𝑖 = 𝒙̈ + 𝝎̇ × 𝒓𝑖 + 𝝎 × 𝝎 × 𝒓𝑖,
𝝎̇𝑖 = 𝝎̇,
which can be inserted into (28.9)-(28.10) to yield 
𝑚𝑖[𝒙̈ + 𝝎̇ × 𝒓𝑖] = 𝒇𝑖
𝑥 − 𝑚𝑖𝝎 × 𝝎 × 𝒓𝑖,
𝑱𝑖𝝎̇ = 𝒇𝑖
𝜔 − 𝝎 × 𝑱𝑖𝝎.
This can be compactly written as 
[
𝑚𝑖 −𝑚𝑖𝑹𝑖
𝑱𝑖
] [ 𝒙̈
𝝎̇
] = [
𝑥 − 𝑚𝑖𝝎 × 𝝎 × 𝒓𝑖
𝒇𝑖
𝜔 − 𝝎 × 𝑱𝑖𝝎
𝒇𝑖
].
(28.11)
(28.12)
(28.13)
(28.14)
(28.15)
It remains to use the principle of virtual work, employing (28.8), to reduce the number 
of equations (rigid body and slave nodes) to the generalized rigid body equations.  The 
result of this endeavor is 
(𝑀𝜌 + ∑ 𝑚𝑖
𝑖∈𝑆
)𝒙̈ − (∑ 𝑚𝑖𝑹𝑖
𝑖∈𝑆
)𝝎̇ = 𝒇𝜌
𝑥 + ∑ (𝒇𝑖
𝑥 − 𝑚𝑖𝝎 × 𝝎 × 𝒓𝑖)
𝑖∈𝑆
, 
(28.16)
−(∑ 𝑚𝑖𝑹𝑖
𝑖∈𝑆
)𝒙̈ + (𝑱𝜌 + ∑ 𝑱𝑖
𝜔 + ∑ (𝒇𝑖
+ ∑ 𝑚𝑖𝑹𝑖
𝑖∈𝑆
𝑖∈𝑆
𝜔 − 𝝎 × 𝑱𝑖𝝎)
= 𝒇𝜌
)𝝎̇
𝑇𝑹𝑖
− ∑ 𝑹𝑖
𝑖∈𝑆
𝑖∈𝑆
𝑇(𝒇𝑖
𝑥 − 𝑚𝑖𝝎 × 𝝎 × 𝒓𝑖)
− 𝝎 × 𝑱𝜌𝝎,
(28.17)
A simplified expression can be obtained through the variable substitution 
𝒛 = 𝒙 +
∑ 𝑚𝑖𝒓𝑖
𝑖∈𝑆
.
(28.18)
This yields 𝒙̈ = 𝒛̈ + 𝑹𝑧−𝑥𝝎̇ − 𝝎 × 𝝎 × 𝒓𝑧−𝑥 where 𝒓𝑧−𝑥 = 𝒛 − 𝒙  and 𝑹𝑧−𝑥𝒓 = 𝒓𝑧−𝑥 × 𝒓 for an 
arbitrary vector 𝒓. This can be inserted into (28.16) and (28.17) to provide 
where 
𝑀𝒛̈ = 𝒇 𝑥,
𝑱𝝎̇ = 𝒇 𝜔.
𝑀 = 𝑀𝜌 + ∑ 𝑚𝑖
𝑖∈𝑆
,
𝒇 𝑥 = 𝒇𝜌
𝑥 + ∑ 𝒇𝑖
𝑖∈𝑆
,
𝑱 = 𝑱𝜌 + ∑ 𝑱𝑖
𝑖∈𝑆
+ ∑ 𝑚𝑖𝑹𝑖
𝑖∈𝑆
𝑇𝑹𝑖
− 𝑀𝑹𝑧−𝑥
𝑇 𝑹𝑧−𝑥,
(28.19)
(28.20)
(28.21)
(28.22)
(28.23)
Rigid Body Dynamics 
LS-DYNA Theory Manual 
𝒇 𝜔 =   −𝝎 × 𝑱𝝎 + 𝒇𝜌
𝜔 + ∑ (𝒇𝑖
𝜔 + 𝒓𝑖 × 𝒇𝑖
𝑥)
𝑖∈𝑆
− 𝒓𝑧−𝑥 × 𝒇 𝑥. 
(28.24)
Equations  (28.19)-(28.24)  are  the  generalized  rigid  body  equations  to  be  solved 
for 𝒙 and 𝑸, cf. (28.5) and (28.18). The mass in (28.21) and inertia tensor in (28.23) are the 
physical  mass and  physical inertia augmented by slave node properties; nodal masses 
𝑚𝑖, inertias 𝑱𝑖 and locations 𝒙𝑖. We denote 𝑀 the algorithmic mass, which may not reflect 
what  the  user  intuitively  expects  when  using  *MAT_RIGID  to  make  a  part  rigid.  
Similarly  𝑱  is  the  algorithmic  inertia  tensor,  and  it  is  worth  noting  that  a  nodal  rigid 
body must therefore be connected to deformable elements or otherwise 𝑀 = 0 and 𝑱 = 𝟎 
and  its  whereabouts  will  be  impossible  to  determine.    For  no  mass  scaling,  all  these 
properties  are  constant  (except  for  rotational  updates  of  the  inertia  tensors)  and  can 
essentially be calculated at time zero.  If mass scaling is active, the slave nodal masses 
and inertias include the added mass due to mass scaling and therefore change over time.  
This means that inertia properties should be recomputed every time step to account for 
these  changes,  but  the  default  behavior  is  that  this  is  done  only  for  nodal  rigid  bodies 
and not for regular rigid bodies.  Presumably this is based on the assumption that the 
influence  from  slave  nodes  is  significant  for  nodal  rigid  bodies  and  not  so  much  for 
regular rigid bodies, which is probably true as long as the number of contiguous nodes 
is  small  compared  to  the  total  number of  nodes  in  the  rigid  body.   Nevertheless,  with 
RBSMS = 1 on *CONTROL_RIGID, these extra masses are accounted for and equations 
(28.19)-(28.24)  are  solved  as  expressed  herein.    This  amounts  to  transforming  𝒙  to  𝒛 
before the update, then update 𝒛, and transform back to obtain the new 𝒙. As we now 
turn  to  the  algorithmic  update  of  the  rigid  body  location,  we  restrict  ourselves  to  a 
special case for the sake of simplifying the exposition; 
1.We neglect mass scaling. 
2.Physical properties are not defined by *PART_INERTIA. 
3.The rigid body is not connected to deformable elements. 
4.No lumped masses are present. 
which means that 𝒛 = 𝒙. 
From (28.19)-(28.20) can readily solve for the rigid body accelerations 
𝒇 𝑥
𝒙̈ =
,
It turns out that the algorithmic mass 𝑀 can be calculated as 
𝝎̇ = 𝑱−1 𝒇 𝜔.
𝑀 = ∑ 𝑀𝑖
𝑖∈𝑆
,
(28.25)
(28.26)
(28.27)
LS-DYNA Theory Manual 
Rigid Body Dynamics 
where  𝑀𝑖  is  the  mass  of  node  𝑖  as  obtained  from  the  mass  of  its  associated  elements 
(integrating  material  density  𝜌  by  shape  functions  𝜑𝑖  over  element  domain).  
Furthermore 𝒙 can be approximated from 
𝑀𝒙 = ∑ 𝑀𝑖𝒙𝑖
𝑖∈𝑆
.
(28.28)
Likewise, the inertia tensor is approximated by a nodal summation of the product of the 
point masses with their moment arms 
𝑱 = ∑ 𝑀𝑖𝑹𝑖
𝑖∈𝑆
𝑇𝑹𝑖
.
(28.29)
The  initial  velocities  of  the  slave  nodes  are  readily  calculated  for  a  rigid  body  from 
(28.6). For arbitrary orientations of the body, the inertia tensor is transformed each time 
step  based  on  the  incremental  rotations  using  the  standard  rules  of  second-order 
tensors: 
𝑱𝑛+1 = 𝑨𝑱𝑛𝑨𝑇
(28.30)
where  𝑱𝑛+1  is  the  updated  inertia  tensor  components  in  the  global  frame.    The 
transformation  matrix  𝑨  is  not  stored  since  the  formulation  is  incremental,  but 
recomputed  as  explained  below.    After  calculating  the  rigid  body  accelerations  from 
Equation  (28.25)  and  (28.26),  the  rigid  body  translational  and  rotational  increment,  ∆𝒙 
and  ∆𝜽,  can  be  calculated  using  the  time  step  ∆𝑡  and  the  explicit  time  integration 
update.  The translational coordinate is then updated as 
and ∆𝜽 is used to calculate 𝑨 in (28.30) using the Hughes-Winget algorithm, 
𝒙𝑛+1 = 𝒙𝑛 + ∆𝒙
𝑨 = 𝑰 +
1 + ∆𝜽𝑇∆𝜽
(𝑰 +
𝛥𝑺) 𝛥𝑺,
𝛥𝑺𝒓 = ∆𝜽 × 𝒓, ∀𝒓.
The coordinates of the slave nodes are incrementally updated 
𝑛+1 = 𝒙𝑖
𝒙𝑖
𝑛,
𝑛 + ∆𝒙 + (𝑨 − 𝑰)𝒓𝑖
and the velocities of the nodes are calculated by differencing the coordinates 
𝒙̇𝑖 =
(𝒙𝑖
𝑛+1 − 𝒙𝑖
𝛥𝑡
𝑛)
.
(28.31)
(28.32)
(28.33)
(28.34)
(28.35)
A  direct  integration  of  the  rigid  body  accelerations  into  velocity  and  displacements  is 
not  used  for  two  reasons:    (1)  calculating  the  rigid  body  accelerations  of  the  nodes  is 
more  expensive  than  the  current  algorithm,  and  (2)  the  second-order  accuracy  of  the 
central difference integration method would introduce distortion into the rigid bodies.  
Since  the  accelerations  are  not  needed  within  the  program,  they  are  calculated  by  a 
post-processor using a difference scheme similar to the above.
Rigid Body Dynamics 
LS-DYNA Theory Manual 
28.1  Rigid Body Joints 
28.1.1  Penalty types 
The joints for the rigid bodies in LS-DYNA, see Figure 28.1, are implemented using the 
penalty method.  Given a constraint equation 𝐶(𝑥𝑖, 𝑥𝑗) = 0, for nodes 𝑖 and 𝑗, the penalty 
function added to the Lagrangian of the system is −1/2𝑘𝐶2(𝑥𝑖, 𝑥𝑗).  The resulting nodal 
forces are: 
𝑓𝑖 = −𝑘𝐶(𝑥𝑖, 𝑥𝑗)
𝑓𝑗 = −𝑘𝐶(𝑥𝑖, 𝑥𝑗)
∂𝐶(𝑥𝑖, 𝑥𝑗)
,
∂𝑥𝑖
∂𝐶(𝑥𝑖, 𝑥𝑗)
.
∂𝑥𝑗
(28.36)
(28.37)
The  forces  acting  at  the  nodes  have  to  convert  into  forces  acting  on  the  rigid 
bodies.  Recall that velocities of a node i is related to the velocity of the center of mass of 
a rigid body by Equation (28.6).  By using Equation (28.6) and virtual power arguments, 
it may be shown that the generalized forces are: 
𝑥 = 𝑓𝑖,
𝐹𝑖
𝜔 = 𝑒𝑖𝑗𝑘𝑥̅𝑗𝑓𝑘,
𝐹𝑖
(28.38)
(28.39)
which are the forces and moments about the center of mass. 
The magnitude of the penalty stiffness 𝑘 is chosen so that it does not control the 
stable  time  step  size.    For  the  central  difference  method,  the  stable  time  step  Δ𝑡  is 
restricted by the condition that, 
Δ𝑡 =
,
(28.40)
where  𝛺  is  the  highest  frequency  in  the  system.    The  six  vibrational  frequencies 
associated  with  each  rigid  body  are  determined  by  solving  their  eigenvalue  problems 
assuming 𝑘 = 1.  For a body with 𝑚 constraint equations, the linearized equations of the 
translational degrees of freedom are  
𝑀𝑋̈ + 𝑚𝑘𝑋 = 0,
(28.41)
and the frequency is √𝑚𝑘/𝑀 where 𝑀 is the mass of the rigid body.  The corresponding 
rotational equations are  
𝐉𝛉̈ + 𝐊𝛉 = 0,
(28.42)
𝐉 is the inertia tensor and 𝐊 is the stiffness matrix for the moment contributions from the 
penalty  constraints.    The  stiffness  matrix  is  derived  by  noting  that  the  moment 
contribution of a constraint may be approximated by  
28-6 (Rigid Body Dynamics) 
𝐅𝑥 = −k𝐫𝑖 × (𝛉 × 𝐫𝑖),
LS-DYNA Theory Manual 
Rigid Body Dynamics 
and noting the identity,  
so that 
𝐫𝑖 = 𝐱𝑖 − 𝐗cm,
𝐀 × (𝐁 × 𝐂) = |𝐀 ⋅ 𝐂 − 𝐀 ⊗ 𝐂|𝐁,
𝐾 = ∑ 𝑘[𝐫𝑖 ⋅ 𝐫𝑖 − 𝐫𝑖 ⊗ 𝐫𝑖]
.
𝑖=1
(28.44)
(28.45)
(28.46)
The rotational frequencies are the roots of the equation det∣𝐊 − 𝛺2𝐉∣ = 0, which is 
cubic in 𝛺2.  Defining the maximum frequency over all rigid bodies for 𝑘 = 1 as 𝛺max, 
and introducing a time step scale factor TSSF, the equation for 𝑘 is 
𝑘 ≤ (
2TSSF
Δ𝑡Ωmax
)
,
(28.47)
The  joint  constraints  are  defined  in  terms  of  the  displacements  of  individual 
nodes.    Regardless  of  whether  the  node  belongs  to  a  solid  element  or  a  structural 
element, only its translational degrees of freedom are used in the constraint equations. 
A spherical joint is defined for nodes 𝑖 and 𝑗 by the three constraint equations, 
𝑥1𝑖 − 𝑥1𝑗 = 0     𝑥2𝑖 − 𝑥2𝑗 = 0
𝑥3𝑖 − 𝑥3𝑗 = 0,
(28.48)
and a revolute joint, which requires five constraints, is defined by two spherical joints, 
for  a  total  of  six  constraint  equations.    Since  a  penalty  formulation  is  used,  the 
redundancy  in  the  joint  constraint  equations  is  unimportant.    A  cylindrical  joint  is 
defined by taking a revolute joint and eliminating the penalty forces along the direction 
defined  by  the  two  spherical  joints.    In  a  similar  manner,  a  planar  joint  is  defined  by 
eliminating the penalty forces that are perpendicular to the two spherical joints.  
The translational joint is a cylindrical joint that permits sliding along its axis, but 
not  rotation.    An  additional  pair  of  nodes  is  required  off  the  axis  to  supply  the 
additional  constraint.    The  only  force  active  between  the  extra  nodes  acts  in  the 
direction normal to the plane defined by the three pairs of nodes. 
The universal joint is defined by four nodes.  Let the nodes on one body be 𝑖 and 
𝑘, and the other body, 𝑗 and 𝑙.  Two of them, 𝑖 and 𝑗, are used to define a spherical joint 
for the first three constraint equations.  The fourth constraint equation is, 
𝐶(𝑥𝑖, 𝑥𝑗, 𝑥𝑘, 𝑥𝑙) = (𝑥𝑘 − 𝑥𝑖) ⋅ (𝑥𝑖 − 𝑥𝑗) = 0,
and  is  differentiated  to  give  the  penalty  forces  𝑓𝑛 = −𝑘𝐶 ∂𝐶
∂𝑥𝑛
four nodes numbers. 
(28.49)
,  where  𝑛  ranges  over  the
Rigid Body Dynamics 
LS-DYNA Theory Manual 
Figure 28.1.  Rigid body joints in LS-DYNA. 
28.1.2  Lagrange multiplier types 
An alternate version of joints is to use constraints and associated Lagrange multipliers.  
To  this  end,  we  recall  the  numerical  update  of  the  rigid  body  kinematics.    Given 
translational and rotational accelerations 𝒙̈ and 𝝎̇, we have 
and 
𝒙̇ = 𝒙̇𝑛 + ∆𝑡𝑛+1/2𝒙̈
𝒙 = 𝒙𝑛 + ∆𝑡𝑛+1𝒙̇
𝝎 = 𝝎𝑛 + ∆𝑡𝑛+1/2𝝎̇
𝑸 = (𝑰 −
−1
∆𝑡𝑛+1𝑹(𝝎))
(𝑰 +
∆𝑡𝑛+1𝑹(𝝎)) 𝑸𝑛
(28.50)
(28.51)
(28.52)
(28.53)
where ∆𝑡𝑛+1/2 = (∆𝑡𝑛+1 + ∆𝑡𝑛)/2 and 𝑹(𝝎)𝒗 = 𝝎 × 𝒗 for an arbitrary vector 𝒗. Here 𝑸 =
[𝒒1 𝒒2 𝒒3]  is  the  orthonormal  system  attached  to  the  rigid  body,  which  we  for 
simplicity  assume  is  aligned  with  whatever joints  we  are  considering.    For  instance,  if 
two bodies 𝑖 and 𝑗 are connected with a joint we let 𝑸𝑖 = 𝑸𝑗 initially, and let the vectors 
are aligned with the axes of the joint.  Also, each body has a point 𝒑 where the system is 
assumed  to  be  attached  and  that  defines  the  origin  of  the  joint.    Referring  to  the  two
LS-DYNA Theory Manual 
Rigid Body Dynamics 
bodies  examplified,  we  assume  that  𝒑𝑖 = 𝒑𝑗  initially.    The  point  𝒑  is  for  simplicity 
expressed  as  𝒑 = 𝒙 + 𝒅,  where  𝒅  is  a  vector  attached  to  the  rigid  body  and  updates  in 
analogy with 𝑸, i.e., using the Hughes-Winget formula (28.53). 
For bodies with no constraints, the accelerations are given directly by the solution of the 
equations of motion for each individual body, but now we seek to solve the equations of 
motion  with  respect  to  the  combined  accelerations  𝑿̈   and  𝜴̇   of  all  bodies  with  joint 
constraints, subject to these constraints.  This can be written as 
𝑴𝑿̈ − 𝑭𝑥 = 𝟎
𝑱𝛀̇ − 𝑭𝜃 = 𝟎
(28.54)
(28.55)
where we have collected quantities for all bodies of interest to form a complete system.  
Here 𝑴 is the mass matrix, 𝑱 is the inertia matrix while 𝑭𝑥 and 𝑭𝜃 are the external forces 
and torques coming from all other features in the model.  The constraints can be written 
and a Lagrangian system is set up as 
𝑪(𝑿̈ , 𝜴̇) = 𝟎,
𝑴𝑿̈ − 𝑭𝑥 + (
)
𝜕𝑪
𝜕𝑿̈
𝜦 = 𝟎
𝑱𝜴̇ − 𝑭𝜃 + (
𝜕𝑪
𝜕𝜴̇
)
𝜦 = 𝟎,
(28.56)
(28.57)
(28.58)
with  𝜦  being  the  Lagrange  multiplier.    In the  quest  for  a  solution, we  linearize  this  to 
form a Newton step according to 
𝑴Δ𝑿̈ +
{⎧
𝜕
𝜕𝑿̈ ⎩{⎨
(
)
Δ𝑿̈ +
𝜕𝑪
𝜕𝑿̈
}⎫
⎭}⎬
= 𝑭𝑥 − 𝑴𝑿̈ − (
{⎧
𝜕
𝜕𝛀̇ ⎩{⎨
𝜕𝑪
𝜕𝑿̈
)
𝜦 
)
(
𝜕𝑪
𝜕𝑿̈
}⎫
⎭}⎬
Δ𝛀̇ + (
𝜕𝑪
𝜕𝑿̈
)
Δ𝜦
𝑱𝛥𝜴̇ +
{⎧
𝜕
𝜕𝑿̈ ⎩{⎨
(
)
𝜕𝑪
𝜕𝜴̇
𝛥𝑿̈ +
}⎫
⎭}⎬
= 𝑭𝜃 − 𝑱𝜴̇ − (
{⎧
𝜕
𝜕𝜴̇ ⎩{⎨
𝜕𝑪
𝜕𝜴̇
)
𝜦. 
)
(
𝜕𝑪
𝜕𝜴̇
}⎫
⎭}⎬
𝛥𝜴̇ + (
𝜕𝑪
𝜕𝜴̇
)
𝛥𝜦
This is accompanied with a linearization of the constraints themselves 
𝜕𝑪
𝜕𝑿̈
𝛥𝑿̈ +
𝜕𝑪
𝜕𝜴̇
𝛥𝜴̇ = −𝑪
(28.59)
(28.60)
(28.61)
to form a solvable system of equations.  Given a starting solution 𝑿̈ = 𝟎, 𝜴̇ = 𝟎, and 𝜦 =
𝟎, the first system to solve is simplified to
Rigid Body Dynamics 
LS-DYNA Theory Manual 
𝑴Δ𝑿̈ + (
𝜕𝑪
𝜕𝑿̈
)
Δ𝜦 = 𝑭𝑥
𝑱𝛥𝜴̇ + (
)
𝜕𝑪
𝜕𝜴̇
𝛥𝜦 = 𝑭𝜃.
(28.62)
(28.63)
This,  i.e.,  equations  (28.61)-(28.63),  is  a  standard  symmetric  Lagrange  system  of 
equations,  and  is  often  sufficient  to  yield  an  accurate  solution  without  iterating.  
However,  due  to  nonlinearity  𝑪  may  grow  and  therefore  a  fully  iterative  scheme  is 
performed according at a time step frequency given by an internal rule.  For simplicity, 
the approximation 𝜦 ≈ 𝟎 is maintained for the setup of the system matrix to avoid the 
second  derivative  of  constraints  and  a  more  complex  nonsymmetric  system.    For  the 
right hand side we make no such approximation.  
Some of the joint constraints of interest are 
Spherical joint 
Revolute joint 
Cylindrical joint 
Planar joint 
𝒑𝑖 − 𝒑𝑗 = 𝟎
𝒑𝑖 − 𝒑𝑗 = 𝟎
𝑖 ∙ 𝒒2
𝒒1
𝑗 = 𝒒3
𝑖 ∙ 𝒒1
𝑗 = 0
𝑖 ∙ (𝒑𝑖 − 𝒑𝑗) = 𝒒3
𝒒2
𝑖 ∙ (𝒑𝑖 − 𝒑𝑗) = 0
𝑖 ∙ 𝒒2
𝒒1
𝑗 = 𝒒3
𝑖 ∙ 𝒒1
𝑗 = 0
𝑖 ∙ (𝒑𝑖 − 𝒑𝑗) = 0
𝒒1
𝑖 ∙ 𝒒2
𝒒1
𝑗 = 𝒒3
𝑖 ∙ 𝒒1
𝑗 = 0
Translational joint 
𝑖 ∙ (𝒑𝑖 − 𝒑𝑗) = 𝒒3
𝒒2
𝑖 ∙ (𝒑𝑖 − 𝒑𝑗) = 0
𝑖 ∙ 𝒒2
𝒒1
𝑗 = 𝒒2
𝑖 ∙ 𝒒3
𝑗 = 𝒒3
𝑖 ∙ 𝒒1
𝑗 = 0
(28.64)
(28.65)
(28.66)
(28.67)
(28.68)
(28.69)
(28.70)
(28.71)
(28.72)
To  form  the  system  of  equations,  the  first  order  sensitivities  needed  are  those  of  𝑸,  𝒙 
and 𝒅, and can be expressed as
LS-DYNA Theory Manual 
Rigid Body Dynamics 
𝛿𝒒𝑖 = ∆𝑡𝑛+1 (𝑰 −
−1
∆𝑡𝑛+1𝑹(𝝎))
𝛿𝝎 ×
≈ ∆𝑡𝑛+1∆𝑡𝑛+1/2𝛿𝝎̇ × 𝒒𝑖
{⎧
⎩{⎨
(𝑰 −
−1
∆𝑡𝑛+1𝑹(𝝎))
𝒒𝑖
}⎫
⎭}⎬
𝛿𝒅 = ⋯ ≈ ∆𝑡𝑛+1∆𝑡𝑛+1/2𝛿𝝎̇ × 𝒅
𝛿𝒙 = ∆𝑡𝑛+1∆𝑡𝑛+1/2𝛿𝒙̈
(28.73)
(28.74)
(28.75)
where  we  have  differentiated  (28.50)-(28.53)  using  the  accelerations  as  independent 
variables. 
28.2  Deformable to Rigid Material Switching 
Occasionally  in  practice,  long  duration,  large  rigid  body  motions  arise  that  are 
prohibitively expensive to simulate if the elements in the model are deformable.  Such a 
case could occur possibly in automotive rollover where the time duration of the rollover 
would dominate the cost relative to the post impact response that occurs much later.  
To  permit  such  simulations  to  be  efficiently  handled  a  capability  to  switch  a 
subset  of  materials  from  deformable  to  rigid  and  back  to  deformable  is  available.    In 
practice the suspension system and tires would remain deformable A flag is set in the 
input to let LS-DYNA know that all materials in the model have the potential to become 
rigid  bodies  sometime  during  the  calculation.    When  this  flag  is  set  a  cost  penalty  is 
incurred on vector machines since the blocking of materials in the element loops will be 
based on the part ID rather than the material type ID.  Normally this cost is insignificant 
relative to the cost reduction due to this unique feature. 
For  rigid  body  switching  to  work  properly  the  choice  of  the  shell  element 
formulation  is  critical.    The  Hughes-Liu  elements  cannot  currently  be  used  for  two 
reasons.  First, since these elements compute the strains from the rotations of the nodal 
fiber vectors from one cycle to the next, the nodal fiber vectors should be updated with 
the  rigid  body  motions  and  this  is  not  done.    Secondly,  the  stresses  are  stored  in  the 
global system as opposed to the co-rotational system.  Therefore, the stresses would also 
need  to  be  transformed  with  the  rigid  body  motions  or  zeroed  out.    The  co-rotational 
elements  of  Belytschko  and  co-workers  do  not  reference  nodal  fibers  for  the  strain 
computations  and  the  stresses  are  stored  in  the  co-rotational  coordinate  system  which 
eliminates the need for the transformations; consequently, these elements can be safely 
used.  The membrane elements and airbag elements are closely related to the Belytschko 
shells and can be safely used with the switching options. 
The  beam  elements  have  nodal  triads  that  are  used  to  track  the  nodal  rotations 
and to calculate the deformation displacements from one cycle to the next.  These nodal 
triads  are  updated  every  cycle  with  the  rigid  body  rotations  to  prevent  non-physical
Rigid Body Dynamics 
LS-DYNA Theory Manual 
behavior when the rigid body is switched back to deformable.  This applies to all beam 
element  formulations  in  LS-DYNA.    The  Belytschko  beam  formulations  are  preferred 
for  the  switching  options  for  like  the  shell  elements,  the  Hughes-Liu  beams  keep  the 
stresses in the global system.  Truss elements like the membrane elements are trivially 
treated and pose no difficulties. 
The brick elements store the stresses in the global system and upon switching the 
rigid  material  to  deformable  the  element  stresses  are  zeroed  to  eliminate  spurious 
behavior. 
The  implementation  addresses  many  potential  problems  and  has  worked  well  in 
practice.    The  current  restrictions  can  be  eliminated  if  the  need  arises  and  anyway 
should pose no insurmountable problems.  We will continue to improve this capability 
if we find that it is becoming a popular option. 
28.3  Rigid Body Welds 
The weld capability in LS-DYNA is based on rigid body dynamics.  Each weld is 
defined by a set of nodal points which moves rigidly with six degrees of freedom until a 
failure criteria is satisfied.  Five weld options are implemented including: 
•Spot weld. 
•Fillet weld 
•Butt weld 
•Cross fillet weld 
•General weld 
Welds  can  fail  three  ways:  by  ductile  failure  which  is  based  on  the  effective 
plastic strain, by brittle failure which is based on the force resultants acting on the rigid 
body weld, and by a failure time which is specified in the input.  When effective plastic 
strain  is  used  the  weld  fails  when  the  nodal  plastic  strain  exceeds  the  input  value.    A 
least  squares  algorithm  is  used  to  generate  the  nodal  values  of  plastic  strains  at  the 
nodes  from  the  element  integration  point  values.    The  plastic  strain  is  integrated 
through the element and the average value is projected to the nodes with a least square 
fit.  In the resultant based brittle failure the resultant forces and moments on each node 
of  the  weld  are  computed.    These  resultants  are  checked  against  a  failure  criterion 
which is expressed in terms of these resultants.  The forces may be averaged over a user 
specified  number  of  time  steps  to  eliminate  breakage  due  to  spurious  noise.    After  all 
nodes of a weld are released the rigid body is removed from the calculation.
LS-DYNA Theory Manual 
Rigid Body Dynamics 
node 2
node 1
node 3
node 2
2 node spotweld
3 node spotweld
node 1
node n
node n-1
n node spotweld
node 2
node 1
Figure 28.2.  Nodal ordering and orientation of the local coordinate system is
important for determining spotweld failure. 
Spotwelds  are  shown  in  Figure  28.2.    Spotweld  failure  due  to  plastic  straining 
p .  This option 
occurs when the effective nodal plastic strain exceeds the input value, 𝜀fail
can  model  the  tearing  out  of  a  spotweld  from  the  sheet  metal  since  the  plasticity  is  in 
the material that surrounds the spotweld, not the spotweld itself.   This option should 
only  be  used  for  the  material  models  related  to  metallic  plasticity  and  can  result  is 
slightly increased run times. 
Brittle failure of the spotwelds occurs when: 
(
max(𝑓𝑛, 0)
𝑆𝑛
)
+ (
∣𝑓𝑠∣
𝑆𝑠
)
≥ 1,
(28.76)
where 𝑓𝑛 and 𝑓𝑠 are the normal and shear interface force.  Component 𝑓𝑛 contributes for 
tensile values only.  When the failure time, 𝑡f, is reached the nodal rigid body becomes
Rigid Body Dynamics 
LS-DYNA Theory Manual 
inactive and the constrained nodes may move freely.  In Figure 28.2 the ordering of the 
nodes is shown for the 2 and 3 noded spotwelds.  This order is with respect to the local 
coordinate system where the local 𝑧 axis determines the tensile direction.  The nodes in 
the spotweld may coincide but if they are offset the local system is not needed since the 
𝑧-axis is automatically oriented based on the locations of node 1, the origin, and node 2.  
The failure of the 3 noded spotweld may occur gradually with first one node failing and 
later  the  second  node  may  fail.    For  𝑛  noded  spotwelds  the  failure  is  progressive 
starting with the outer nodes (1 and 𝑛) and then moving inward to nodes 2 and 𝑛 − 1.  
Progressive failure is necessary to preclude failures that would create new rigid bodies. 
Ductile  fillet  weld  failure,  due  to  plastic  straining,  is  treated  identically  to 
spotweld failure.  Brittle failure of the fillet welds occurs when: 
𝛽√𝜎𝑛
2 + 3(𝜏𝑛
2 + 𝜏𝑡
2) ≥ 𝜎𝑓 ,
(28.77)
where 
𝜎𝑛 = normal stress 
𝜏𝑛 = shear stress in direction of weld (local 𝑦) 
𝜏𝑡 = shear stress normal to weld (local 𝑥) 
𝜎𝑓 = failure stress 
𝛽 = failure parameter 
Component  𝜎𝑛  is  nonzero  for  tensile  values  only.    When  the  failure  time,  𝑡𝑓 ,  is 
reached  the  nodal  rigid  body  becomes  inactive  and  the  constrained  nodes  may  move 
local coordinate
system
2 node fillet weld
3 node fillet weld
Figure 28.3.  Nodal ordering and orientation of the local coordinate system is
shown for fillet weld failure. 
28-14 (Rigid Body Dynamics)
LS-DYNA Theory Manual 
Rigid Body Dynamics 
z1
y1
x1
y2
z2
x2
z3 x3
y3
Figure  28.5.    A  simple  cross  fillet  weld  illustrates  the  required  input.    Here
NFW = 3 with nodal pairs (A = 2, B = 1), (A = 3, B = 1), and (A = 3, B = 2).  The 
local coordinate axes are shown.  These axes are fixed in the rigid body and are 
referenced  to  the  local  rigid  body  coordinate  system  which  tracks  the  rigid
body rotation. 
freely.  In Figure 28.3 the ordering of the nodes is shown for the 2 node and 3 node fillet 
welds.  This order is with respect to the local coordinate system where the local z axis 
determines the tensile direction.  The nodes in the fillet weld may coincide.  The failure 
of  the  3  node  fillet  weld  may  occur  gradually  with  first  one  node failing  and  later  the 
second node may fail.   
In  Figure  28.4  the  butt  weld  is  shown.    Ductile  butt  weld  failure,  due  to  plastic 
straining,  is  treated  identically  to  spotweld  failure.    Brittle  failure  of  the  butt  welds 
occurs when: 
𝛽√𝜎𝑛
2 + 3(𝜏𝑛
2 + 𝜏𝑡
2) ≥ 𝜎𝑓 ,
(28.78)
where 
𝜎𝑛 = normal stress 
𝜏𝑛 = shear stress in direction of weld (local y) 
𝜏𝑡 = shear stress normal to weld (local z) 
𝜎𝑓 = failure stress 
𝛽 = failure parameter 
Component 𝜎𝑛 is nonzero for tensile values only.  When the failure time, 𝑡𝑓  , is reached 
the nodal rigid body becomes inactive and the constrained nodes may move freely.  The 
nodes in the butt weld may coincide.
Rigid Body Dynamics 
LS-DYNA Theory Manual 
The  cross  fillet  weld  and  general  weld  are  shown  in  Figures  28.5  and  28.6, 
respectively.    The  treatment  of  failure  for  these  welds  is  based  on  the  formulation  for 
the fillet and butt welds. 
Figure 28.6.  A general weld is a mixture of fillet and butt welds.
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
29    
Contact-Impact Algorithm 
29.1  Introduction 
The  treatment  of  sliding  and  impact  along  interfaces  has  always  been  an 
important  capability  in  DYNA3D  and  more  recently  in  LS-DYNA.    Three  distinct 
methods  for  handling  this  have  been  implemented,  which  we  will  refer  to  as  the 
kinematic  constraint  method,  the  penalty  method,  and  the  distributed  parameter 
method.    Of  these,  the  first  approach  is  now  used  for  tying  interfaces.    The  relative 
merits of each approach are discussed below. 
Interfaces  can  be  defined  in  three  dimensions  by  listing  in  arbitrary  order  all 
triangular and quadrilateral segments that comprise each side of the interface.  One side 
of the interface is designated as the slave side, and the other is designated as the master 
side.    Nodes  lying  in  those  surfaces  are  referred  to  as  slave  and  master  nodes, 
respectively.  In the symmetric penalty method, this distinction is irrelevant, but in the 
other  methods  the  slave  nodes  are  constrained  to  slide  on  the  master  surface  after 
impact  and  must  remain  on  the  master  surface  until  a  tensile  force  develops  between 
the node and the surface. 
Today,  automatic  contact  definitions  are  commonly  used.    In  this  approach  the 
slave and master surfaces are generated internally within LS-DYNA from the part ID's 
given for each surface.  For automotive crash models it is quite common to include the 
entire  vehicle  in  one  single  surface  contact  definition  where  the  all  the  nodes  and 
elements within the interface can interact. 
29.2  Kinematic Constraint Method 
The kinematic constraint method which uses the impact and release conditions of 
Hughes  et  al.,  [1976]  was  implemented  first  in  DYNA2D  [Hallquist  1976b]  and  finally
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
extended  to  three  dimensions  in  DYNA3D.    Constraints  are  imposed  on  the  global 
equations by a transformation of the nodal displacement components of the slave nodes 
along the contact interface.  This transformation has the effect of eliminating the normal 
degree of freedom of nodes.  To preserve the efficiency of the explicit time integration, 
the mass is lumped to the extent that only the global degrees of freedom of each master 
node  are  coupled.    Impact  and  release  conditions  are  imposed  to  insure  momentum 
conservation.    The  release  conditions  are  of  academic  interest  and  were  quickly 
removed from the coding. 
Problems arise with this method when the master surface zoning is finer than the 
slave surface zoning as shown in two dimensions in Figure 29.1.  Here, certain master 
nodes  can  penetrate  through  the  slave  surface  without  resistance  and  create  a  kink  in 
the  slide  line.    Such  kinks  are  relatively  common  with  this  formulation,  and,  when 
interface pressures are high, these kinks occur whether one or more quadrature points 
are  used  in  the  element  integration.    It  may  be  argued,  of  course,  that  better  zoning 
would  minimize  such  problems;  but  for  many  problems  that  are  of  interest,  good 
zoning in the initial configuration may be very poor zoning later.  Such is the case, for 
example, when gaseous products of a high explosive gas expand against the surface of a 
structural member. 
29.3  Penalty Method 
The penalty method is used in the explicit programs DYNA2D and DYNA3D as 
well as in the implicit programs NIKE2D and NIKE3D.  The method consists of placing 
normal  interface  springs  between  all  penetrating  nodes  and  the  contact  surface.    With 
the  exception  of  the  spring  stiffness  matrix  which  must  be  assembled  into  the  global 
stiffness  matrix, the implicit and explicit treatments are similar.  The NIKE2D/3D and 
DYNA2D/3D programs compute a unique modulus for the element in which it resides.  
In  our  opinion,  pre-empting  user  control  over  this  critical  parameter  greatly  increases 
slave surface
master surface
Indicates nodes treated as free surface nodes
Figure  29.1.    Nodes  of  the  master  slide  surface  designated  with  an  “x”  are 
treated as free surface nodes in the nodal constraint method. 
the success of the method.
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
Quite in contrast to the nodal constraint method, the penalty method approach is 
found  to  excite  little  if  any  mesh  hourglassing.    This  lack  of  noise  is  undoubtedly 
attributable to the symmetry of the approach.  Momentum is exactly conserved without 
the  necessity  of  imposing  impact  and  release  conditions.    Furthermore,  no  special 
treatment of intersecting interfaces is required, greatly simplifying the implementation. 
Currently three implementations of the penalty algorithm are available:   
•  Standard Penalty Formulation 
•  Soft  Constraint  Penalty  Formulation,  which  has  been  implemented  to  treat 
contact  between  bodies  with  dissimilar  material  properties  (e.g.  steel-foam).  
Stiffness calculation and its update during the simulation differs from the Stand-
ard Penalty Formulation.   
•  Segment-based  Penalty  Formulation,  it  is  a  powerful  contact  algorithm  whose 
logic  is  a  slave  segment-master  segment  approach  instead  of  a  traditional  slave 
node-master segment approach.  This contact has proven very useful for airbag 
self-contact during inflation and complex contact conditions.    
In  the  standard  penalty  formulation,  the  interface  stiffness  is  chosen  to  be 
approximately  the  same  order  of  magnitude  as  the  stiffness  of  the  interface  element 
normal to the interface.  Consequently the computed time step size is unaffected by the 
existence of the interfaces.  However, if interface pressures become large, unacceptable 
penetration may occur.  By scaling up the stiffness and scaling down the time step size, 
we may still solve such problems using the penalty approach.  Since this increases the 
number  of  time  steps and  hence  the  cost,  a sliding-only  option  has  been  implemented 
for  treating  explosive-structure  interaction  problems  thereby  avoiding  use  of  the 
penalty  approach.    This  latter  option  is  based  on  a  specialization  of  the  third  method 
described below. 
29.4  Distributed Parameter Method 
This  method  is  used  in  DYNA2D,  and  a  specialization  of  it  is  the  sliding  only 
option in DYNA3D.  Motivation for this approach came from the TENSOR [Burton et.  
al., 1982] and HEMP [Wilkins 1964] programs which displayed fewer mesh instabilities 
than DYNA2D with the nodal constraint algorithm.  The first DYNA2D implementation 
of  this  last  algorithm  is  described  in  detail  by  Hallquist  [1978].    Since  this  early 
publication, the method has been moderately improved but the major ideas remain the 
same.
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
b1
∂b1
∂b2
b2
∂B1
B1
∂B2
B2
Figure 29.2.  Reference and deformed configuration. 
In the distributed parameter formulation, one-half the slave element mass of each 
element in contact is distributed to the covered master surface area.  Also, the internal 
stress  in  each  element  determines  a  pressure  distribution  for  the  master  surface  area 
that receives the mass.  After completing this distribution of mass and pressure, we can 
update  the  acceleration  of  the  master  surface.    Constraints  are  then  imposed  on  slave 
node  accelerations  and  velocities  to  insure  their  movement  along  the  master  surface.  
Unlike the finite difference hydro programs, we do not allow slave nodes to penetrate; 
therefore we avoid “put back on” logic.  In another simplification, our calculation of the 
slave element relative volume ignores any intrusion of the master surfaces.  The HEMP 
and TENSOR codes consider the master surface in this calculation. 
29.5  Preliminaries 
Consider the time-dependent motion of two bodies occupying regions B1 and B2 
in their undeformed configuration at time zero.  Assume that the intersection 
B1 ∩ B2 = 0,
(29.1)
is satisfied.  Let 𝜕B1 and ∂B2denote the boundaries of B1 and B2, respectively.  At some 
later time, these bodies occupy regions b1 and b2 bounded by ∂b1and  ∂b2as shown in 
Figure 29.2.  Because the deformed configurations cannot penetrate, 
(b1 − ∂b1) ∩ b2 = 0.
(29.2)
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
S1
ns
S2
S4
ms
S3
X3
X2
X1
Figure  29.3.    In  this  figure,  four  master  segments  can  harbor  slave  node  𝑛𝑠
given that 𝑚𝑠 is the nearest master node. 
As  long  as  (∂b1 ∩ ∂b2) = 0,  the  equations  of  motion  remain  uncoupled.    In  the 
foregoing  and  following  equations,  the  right  superscript 𝛼  (= 1,2)  denotes  the  body  to 
which the quantity refers. 
Before  a  detailed  description  of  the  theory  is  given,  some  additional  statements 
should  be  made  concerning  the  terminology.    The  surfaces  ∂b1  and  ∂b2  of  the 
discretized bodies b1 and b2 become the master and slave surfaces respectively.  Choice 
of  the  master  and  slave  surfaces  is  arbitrary  when  the  symmetric  penalty  treatment  is 
employed.    Otherwise,  the  more  coarsely  meshed  surface  should  be  chosen  as  the 
master surface unless there is a large difference in mass densities in which case the side 
corresponding to the material with the highest density is recommended.  Nodal points 
that define ∂b1 are called master nodes and nodes that define ∂b2 are called slave nodes.  
When  (∂b1 ∩ ∂b2) ≠ 0,  the  constraints  are  imposed  to  prevent  penetration.    Right 
superscripts are implied whenever a variable refers to either the master surface ∂b1, or 
slave  surface,  ∂b2;  consequently,  these  superscripts  are  dropped  in  the  development 
which follows. 
29.6  Slave Search 
The  slave  search  is  common  to  all  interface  algorithms  implemented  in 
DYNA3D.  This search finds for each slave node its nearest point on the master surface.  
Lines drawn from a slave node to its nearest point will be perpendicular to the master 
surface,  unless  the  point  lies  along  the  intersection  of  two  master  segments,  where  a 
segment is defined to be a 3- or 4-node element of a surface.
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
Consider  a  slave  node,  𝑛𝑠,  sliding  on  a  piecewise  smooth  master  surface  and 
assume that a search of the master surface has located the master node, 𝑚𝑠, lying nearest 
to 𝑛𝑠.  Figure 29.3 depicts a portion of a master surface with nodes 𝑚𝑠 and 𝑛𝑠 labeled.  If 
𝑚𝑠  and  𝑛𝑠  do  not  coincide,  𝑛𝑠  can  usually  be  shown  to  lie  in  a  segment  𝑠1  via  the 
following tests: 
(𝐜𝑖 × 𝐬) ⋅ (𝐜𝑖 × 𝐜𝑖+1) > 0,
(𝐜𝑖 × 𝐬) ⋅ (𝐬 × 𝐜𝑖+1) > 0,
(29.3)
where vector 𝐜𝑖 and 𝐜𝑖+1 are along edges of 𝑠1 and point outward from 𝑚𝑠.  Vector 𝐬 is 
the  projection  of  the  vector  beginning  at  𝑚𝑠,  ending  at  𝑛𝑠,  and  denoted  by  𝐠,  onto  the 
plane being examined . 
where for segment 𝑠1 
𝐬 = 𝐠 − (𝐠 ⋅ 𝐦)𝐦,
𝐦 =
𝐜𝑖 × 𝐜𝑖+1
∣𝐜𝑖 × 𝐜𝑖+1∣
.
(29.4)
(29.5)
Since  the  sliding  constraints  keep  𝑛𝑠  close  but  not  necessarily  on  the  master 
surface  and  since  𝑛𝑠  may  lie  near  or  even  on  the  intersection  of  two  master  segments, 
the inequalities of Equation (29.3) may be inconclusive, i.e., they may fail to be satisfied 
or more than one may give positive results.  When this occurs 𝑛𝑠 is assumed to lie along 
the intersection which yields the maximum value for the quantity 
𝐠 ⋅ 𝐜𝑖
|𝐜𝑖|
𝑖 = 1,2,3,4, ..
(29.6)
When the contact surface is made up of badly shaped elements, the segment apparently 
identified as containing the slave node actually may not, as shown in Figure 29.5.  
ns
ci+1
ms
X3
X2
X1
Figure 29.4.  Projection of g onto master segment 𝑠1
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
Figure 29.5.  When the nearest node fails to contain the segment that harbors
the slave node, segments numbered 1-8 are searched in the order shown. 
Assume that a master segment has been located for slave node 𝑛𝑠 and that 𝑛𝑠 is 
not  identified  as  lying  on  the  intersection  of  two  master  segments.    Then  the 
identification of the contact point, defined as the point on the master segment which is 
nearest  to  𝑛𝑠,  becomes  nontrivial.    For  each  master  surface  segment,  𝑠1  is  given  the 
parametric representation of Equation (1.7), repeated here for clarity: 
where 
𝐫 = 𝑓1(𝜉 , 𝜂)𝐢1 + 𝑓2(𝜉 , 𝜂)𝐢2 + 𝑓3(𝜉 , 𝜂)𝐢3,
𝑓𝑖(𝜉 , 𝜂) = ∑ 𝜙𝑗𝑥𝑖
.
𝑗=1
Note that r1 is at least once continuously differentiable and that 
∂𝐫
∂𝜉
×
∂𝐫
∂𝜂
≠ 0,
(29.7)
(29.8)
(29.9)
Thus 𝐫 represents a master segment that has a unique normal whose direction depends 
continuously on the points of s1. 
Let  t  be  a  position  vector  drawn  to  slave  node  ns  and  assume  that  the  master 
surface segment s1 has been identified with ns.  The contact point coordinates (𝜉c, 𝜂c) on 
s1 must satisfy 
∂𝐫
∂𝜉
∂𝐫
∂𝜂
(𝜉𝑐, 𝜂𝑐) ⋅ [𝐭 − 𝐫(𝜉𝑐, 𝜂𝑐)] = 0,
(𝜉𝑐, 𝜂𝑐) ⋅ [𝐭 − 𝐫(𝜉𝑐, 𝜂𝑐)] = 0.
(29.10)
(29.11)
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
ns
X3
X2
X1
  Figure 29.6.  Location of contact point when ns lies above master segment. 
The  physical  problem  is  illustrated  in  Figure  29.6,  which  shows  ns  lying  above 
the master surface.  Equations (29.10) and (29.11) are readily solved for 𝜉c and  𝜂c.  One 
way to accomplish this is to solve Equation (29.10) for 𝜉c in terms of 𝜂c, and substitute 
the results into Equation (29.11).  This yields a cubic equation in 𝜂c which is presently 
solved  numerically  in  LS-DYNA.    In  the  near  future,  we  hope  to  implement  a  closed 
form solution for the contact point. 
The  equations  are  solved  numerically. 
  When  two  nodes  of  a  bilinear 
quadrilateral  are  collapsed  into  a  single  node  for  a  triangle,  the  Jacobian  of  the 
minimization  problem  is  singular  at  the  collapsed  node.    Fortunately,  there  is  an 
analytical solution for triangular segments since three points define a plane.  Newton-
Raphson iteration is a natural choice for solving these simple nonlinear equations.  The 
method diverges with distorted elements unless the initial guess is accurate.  An exact 
contact point calculation is critical in post-buckling calculations to prevent the solution 
from wandering away from the desired buckling mode.   
Three  iterations  with  a  least-squares  projection  are  used  to  generate  an  initial 
guess: 
[
𝜉0 = 0,         𝜂0 = 0,
𝐫,𝜉
𝐫,𝜂
𝜉𝑖+1 = 𝜉𝑖 + Δ𝜉 ,
] [𝐫,𝜉  𝐫,𝜂] {
Δ𝜉
Δ𝜂
} = [
𝐫,𝜉
𝐫,𝜂
] {𝐫(𝜉𝑖,𝜂𝑖) − 𝐭}, 
(29.12)
𝜂𝑖+1 = 𝜂𝑖 + Δ𝜂,
followed  by  the  Newton-Raphson  iterations  which  are  limited  to  ten  iterations,  but 
which usually converges in four or less.
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
[H] {
Δ𝜉
Δ𝜂
} = − {
𝐫,𝜉
𝐫,𝜂
[H] = {
𝐫,ξ
𝐫,η
} [𝐫,𝜉  𝐫,𝜂] + [
} {𝐫(𝜉𝑖,𝜂𝑖) − 𝐭},
𝐫 ⋅ 𝐫,𝜉𝜂
𝐫 ⋅ 𝐫,𝜉𝜂
] , 
(29.13)
𝜉𝑖+1 = 𝜉𝑖 + Δ𝜉 , 𝜂𝑖+1 = 𝜂𝑖 + Δ𝜂,
In  concave  regions,  a  slave  node  may  have  isoparametric  coordinates  that  lie 
outside of the [−1, +1] range for all of the master segments, yet still have penetrated the 
surface.    A  simple  strategy  is  used  for  handling  this  case,  but  it  can  fail.    The  contact 
segment for each node is saved every time step.  If the slave node contact point defined 
in terms of the isoparametric coordinates of the segment, is just outside of the segment, 
and  the  node  penetrated  the  isoparametric  surface,  and  no  other  segment  associated 
with the nearest neighbor satisfies the inequality test, then the contact point is assumed 
to occur on the edge of the segment.  In effect, the definition of the master segments is 
extended  so  that  they  overlap  by  a  small  amount.    In  the  hydrocode  literature,  this 
approach  is  similar  to  the  slide  line  extensions  used  in  two  dimensions.    This  simple 
procedure  works  well  for  most  cases,  but  it  can  fail  in  situations  involving  sharp 
concave corners. 
29.7  Sliding With Closure and Separation 
29.7.1  Standard Penalty Formulation  
Because this is perhaps the most general and most used interface algorithm, we 
choose to discuss it first.  In applying this penalty method, each slave node is checked 
for  penetration  through  the  master  surface.    If  the  slave  node  does  not  penetrate, 
nothing  is  done.    If  it  does  penetrate,  an  interface  force  is  applied  between  the  slave 
node and its contact point.  The magnitude of this force is proportional to the amount of 
penetration.  This may be thought of as the addition of an interface spring. 
Penetration of the slave node ns through the master segment which contains its 
contact point is indicated if 
where 
𝑙 = 𝐧𝑖 × [𝐭 − 𝐫(𝜉𝑐, 𝜂𝑐)] < 0,
𝐧𝑖 = 𝐧𝑖(𝜉𝑐, 𝜂𝑐)
is normal to the master segment at the contact point. 
(29.14)
(29.15)
If slave node ns has penetrated through master segment 𝑠𝑖, we add an interface 
force vector 𝐟s: 
𝐟𝑠 = −𝑙𝑘𝑖𝐧𝑖
if 𝑙 < 0
(29.16)
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
to the degrees of freedom corresponding to ns and 
𝑖 = 𝜙𝑖(𝜉𝑐, 𝜂𝑐)𝑓𝑠
𝑓𝑚
if 𝑙 < 0
(29.17)
to the four nodes (𝑖 = 1,2,3,4) that comprise master segment 𝑠𝑖.  The stiffness factor 𝑘𝑖 for 
master segment 𝑠𝑖 is given in terms of the bulk modulus 𝐾𝑖, the volume 𝑉𝑖, and the face 
area 𝐴𝑖 of the element that contains 𝑠𝑖 as 
for brick elements and  
𝑘𝑖 =
𝑓𝑠𝑖𝐾𝑖𝐴𝑖
𝑉𝑖
𝑘𝑖 =
𝑓𝑠𝑖𝐾𝑖𝐴𝑖
max(shell  diagonal)
(29.18)
(29.19)
for  shell  elements  where  𝑓𝑠𝑖  is  a  scale  factor  for  the  interface  stiffness  and  is  normally 
defaulted to .10.  Larger values may cause instabilities unless the time step size is scaled 
back in the time step calculation. 
In  LS-DYNA,  a  number  of  options  are  available  for  setting  the  penalty  stiffness 
value.  This is often an issue since the materials in contact may have drastically different 
bulk modulii.  The calculational choices are:  
•  Minimum of the master segment and slave node stiffness.  (default) 
•  Use master segment stiffness 
•  Use slave node value 
•  Use slave node value, area or mass weighted. 
•  As above but inversely proportional to the shell thickness.  
The default may sometimes fail due to an excessively small stiffness.  When this 
occurs it is necessary to manually scale the interface stiffness.  Care must be taken not to 
induce an instability when such scaling is performed.  If the soft material also has a low 
density, it may be necessary to reduce the scale factor on the computed stable time step.   
29.7.2  Soft Constraint Penalty Formulation 
Very soft materials have an undesired effect on the contact stiffness, lowering its 
value and ultimately causing excessive penetration.  An alternative to put a scale factor 
on  the  contact  stiffness  for  SOFT = 0  is  to  use  a  Soft  Constraint  Penalty  Formulation.  
The idea behind this option is to eliminate the excessive penetration by using a different 
formulation for the contact stiffness.  
In  addition  to  the  master  and  slave  contact  stiffness,  an  additional  stiffness  is 
calculated,  which  is  based  on  the  stability  (Courant’s  criterion)  of  the  local  system
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
comprised of two masses (segments) connected by a spring.  This is the stability contact 
stiffness 𝑘cs and is calculated by:  
𝑘cs(𝑡) = 0.5 ⋅ SOFSCL ⋅ 𝑚∗ ⋅ (
,
Δ𝑡𝑐(𝑡)
)
(29.20)
where  SOFSCL  on  Optional  Card  A  of  *CONTROL_CONTACT  is  the  scale  factor  for 
the Soft Constraint Penalty Formulation, 𝑚∗ is a function of the mass of the slave node 
and of the master nodes.  Δ𝑡c is set to the initial solution timestep.  If the solution time 
step grows, Δ𝑡c is reset to the current time step to prevent unstable behavior.   
A comparative check against the contact stiffness calculated with the traditional 
penalty  formulation,  𝑘soft=0,  and  in  general  the  maximum  stiffness  between  the  two  is 
taken,  
𝑘soft=1 = max{𝑘cs, 𝑘soft=0}.
(29.21)
29.7.3  Segment-based Penalty Formulation 
Segment based contact is a general purpose shell and solid element penalty type 
contact  algorithm.    Segment  based  contact  uses  a  contact  stiffness  similar  to  the 
SOFT = 1 stiffness option, but the details are quite different.   
𝑘cs(𝑡) = 0.5 ⋅ SLSFAC ⋅
{⎧SFS
}⎫
or
SFM⎭}⎬
⎩{⎨
(
𝑚1𝑚2
𝑚1 + 𝑚2
) (
)
.
Δ𝑡𝑐(𝑡)
(29.22)
Segment  masses  are  used  rather  than  nodal  masses.    Segment  mass  is  equal  to 
the  element  mass  for  shell  segments  and  half  the  element  mass  for  solid  element 
segments.  Like the Soft Constraint Penalty Formulation, 𝑑𝑡 is set to the initial solution 
time  step  which  is  updated  if  the  solution  time  step  grows  larger  to  prevent  unstable 
behavior.  However, it differs from SOFT = 1 in how 𝑑𝑡 is updated.  𝑑𝑡 is updated only if 
the  solution  time  step  grows  by  more  than  5%.    This  allows  𝑑𝑡  to  remain  constant  in 
most cases, even if the solution time step slightly grows.   
29.8  Recent Improvements in Surface-to-Surface Contact 
A  number  of  recent  changes  have  been  made  in  the  surface-to-surface  contact 
including  contact  searching,  accounting  for  thickness,  and  contact  damping.    These 
changes have been implemented primarily to aid in the analysis of sheet metal forming 
problems.
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
closet nodal point
slave node
Figure 29.7.  Failure to find the contact segment can be caused by poor aspect
ratios in the finite element mesh. 
29.8.1  Improvements to the Contact Searching 
In  metal  forming  applications,  problems  with  the  contact  searching  were  found 
when  the  rigid  body  stamping  dies  were  meshed  with  elements  having  very  poor 
aspect  ratios.    The  nearest  node  algorithm  described  above  can  break  down  since  the 
nearest node is not necessarily anywhere near the segment that harbors the slave node 
as is assumed in Figure 29.5 .  Such  distorted elements are commonly 
used in rigid bodies in order to define the geometry accurately. 
To circumvent the problem caused by bad aspect ratios, an expanded searching 
procedure  is  used  in  which  we  attempt  to  locate  the  nearest  segment  rather  than  the 
nearest  nodal  point.    We  first  sort  the  segments  based  on  their  centroids  as  shown  in 
Figure 29.8 using a one-dimensional bucket sorting technique. 
centroids of master contact segments
search 3 bins for this slave node
Figure  29.8.    One-dimensional  bucket  sorting  identifies  the  nearest  segments 
for each slave node.
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
Figure  29.9.    Interior  points  are  constructed  in  the  segments  for  determining
the closest point to the slave node. 
Once a list of possible candidates is identified for a slave node, it is necessary to 
locate  the  possible  segments  that  contain  the  slave  node  of  interest.    For  each 
quadrilateral segment, four points are constructed at the centroids of the four triangles 
each defined by 3 nodes as shown in Figure 29.9 where the black point is the centroid of 
the quadrilateral.  These centroids are used to find the nearest point to the slave node 
and  hence  the  nearest  segment.    The  nodes  of  the  three  nearest  segments  are  then 
examined  to  identify  the  three  nearest  nodes.    Just  one  node  from  each  segment  is 
allowed to be a nearest node. 
When the nearest segment fails to harbor the slave node, the adjacent segments 
are  checked.    The  old algorithm  checks  the  segments  labeled  1-3  (Figure  29.10),  which 
do not contain the slave node, and fails.  
closet nodal point
slave node
segment identified as containing slave node
Figure 29.10.  In case the stored segment fails to contain the node, the adjacent
segments are checked.
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
Projected contact surface
length of projection vector
is 1/2 the shell thickness
Figure  29.11.    Contact  surface  is  based  on  mid-surface  normal  projection 
vectors. 
29.8.2  Accounting For the Shell Thickness 
Shell thickness effects are important when shell elements are used to model sheet 
metal.  Unless thickness is considered in the contact, the effect of thinning on frictional 
interface stresses due to membrane stretching will be difficult to treat.  In the treatment 
of  thickness  we  project  both  the  slave  and  master  surfaces  based  on  the  mid-surface 
normal  projection  vectors  as  shown  in  Figure  29.11.    The  surfaces,  therefore,  must  be 
offset  by  an  amount  equal  to  1/2  their  total  thickness  (Figure  29.12).    This  allows 
DYNA3D to check the node numbering of the segments automatically to ensure that the 
shells are properly oriented. 
Thickness  changes  in  the  contact  are  accounted  for  if  and  only  if  the  shell 
thickness  change  option  is  flagged  in  the  input.    Each  cycle,  as  the  shell  elements  are 
processed,  the  nodal  thicknesses  are  stored  for  use  in  the  contact  algorithms.    The 
interface stiffness may change with thickness depending on the input options used. 
Figure  29.12.    The  slave  and  master  surfaces  must  be  offset  in  the  input  by
one-half the total shell thickness.  This also allows the segments to be oriented
automatically.
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
Type  5  contact  considers  nodes  interacting  with  a  surface.    This  algorithm  calls 
exactly  the  same  subroutines  as  surface-to-surface  but  not  symmetrically:  i.e.,  the 
subroutines  are  called  once,  not  twice.    To  account  for  the  nodal  thickness,  the 
maximum  shell  thickness  of  any  shell  connected  to  the  node  is  taken  as  the  nodal 
thickness and is updated every cycle.  The projection of the node is done normal to the 
contact surface as shown in Figure 29.13. 
29.8.3  Initial Contact Interpenetrations 
The  need  to  offset  contact  surfaces  to  account  for  the  thickness  of  the  shell 
elements  contributes  to  initial  contact  interpenetrations.    These  interpenetrations  can 
lead to severe numerical problems when execution begins so they should be corrected if 
LS-DYNA  is  to  run  successfully.    Often  an  early  growth  of  negative  contact  energy  is 
one sign that initial interpenetrations exist.  Currently, warning messages are printed to 
the terminal, the D3HSP file, and the MESSAG file to report interpenetrations of nodes 
through contact segments and the modifications to the geometry made by LS-DYNA to 
eliminate the interpenetrations.  Sometimes such corrections simply move the problem 
elsewhere since it is very possible that the physical location of the shell mid-surface and 
possibly  the  shell  thickness  are  incorrect.    In  the  single  surface  contact  algorithms  any 
nodes still interpenetrating on the second time step are removed from the contact with a 
warning message.   
In  some  geometry's  interpenetrations  cannot  be  detected  since  the  contact  node 
interpenetrates completely through the surface at the beginning of the calculation.  This 
is  illustrated  in  Figure  29.14.    Another  case  contributing  to  initial  interpenetrations 
occurs when the edge of a shell element is on the surface of a solid material as seen in 
Figure  29.15.    Currently,  shell  edges  are  rounded  with  a  radius  equal  to  one-half  the 
1/2 thickness of node
Projected contact surface
length of projection vector
is 1/2 the shell thickness
  Figure 29.13.  In a type 5 contact, thickness can also be taken into account. 
shell thickness.
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
Detected Penetration
Undetected Penetration
Figure  29.14.    Undetected  interpenetration.    Such  interpenetrations  are
frequently due to the use of coarse meshes. 
To avoid problems with initial interpenetrations, the following recommendations 
should be considered: 
•Adequately  offset  adjacent  surfaces  to  account  for  part  thickness  during  the 
mesh generation phase. 
•Use consistently refined meshes on adjacent parts which have significant curva-
tures. 
•Be very careful when defining thickness on shell and beam section definitions --
especially for rigid bodies. 
•Scale  back  part  thickness  if  necessary.    Scaling  a  1.5mm  thickness  to  .75mm 
should  not  cause  problems  but  scaling  to  .075mm  might.    Alternatively,  de-
fine  a  smaller  contact  thickness  by  part  ID.    Warning:  if  the  part  is  too  thin 
contact failure will probably occur 
•Use  spot  welds  instead  of  merged  nodes  to  allow  the  shell  mid  surfaces  to  be 
offset. 
29.8.4  Contact Energy Calculation 
Contact  energy,  𝐸contact,  is  incrementally  updated  from  time  𝑛  to  time  𝑛 + 1  for 
each contact interface as: 
Brick
shell
Inner penetration if edge is 
too close
Figure  29.15.    Undetected  interpenetration  due  to  rounding  the  edge  of  the 
shell element.
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
Figure 29.16.  Hemispherical deep drawing problem. 
𝑛+1 = 𝐸contact
𝐸contact
𝑛𝑠𝑛
+ [∑ Δ𝐹𝑖
𝑖=1
slave
× Δ𝑑𝑖𝑠𝑡𝑖
𝑛𝑚𝑛
slave + ∑ Δ𝐹𝑖
𝑖=1
master
𝑛+1
× Δ𝑑𝑖𝑠𝑡𝑖
master]
, 
(29.23)
slave is 
where 𝑛𝑠𝑛 is the number of slave nodes, 𝑛𝑚𝑛 is the number of master nodes, Δ𝐹𝑖
master  is  the 
the  interface  force  between  the  ith  slave  node  and  the  contact  segment  Δ𝐹𝑖
slave  is  the 
interface  force  between  the  ith  master  node  and  the  contact  segment,  Δ𝑑𝑖𝑠𝑡𝑖
incremental  distance  the  ith  slave  node  has  moved  during  the  current  time  step,  and 
master is the incremental distance the ith master node has moved during the current 
Δ𝑑𝑖𝑠𝑡𝑖
time step.  In the absence of friction the slave and master side energies should be close 
in  magnitude  but  opposite  in  sign.    The  sum,  𝐸contact,  should  equal  the  stored  energy.  
Large  negative  contact  energy  is  usually  caused  by  undetected  penetrations.    Contact 
energies  are  reported  in  the  SLEOUT  file.    In  the  presence  of  friction  and  damping 
discussed below the interface energy can take on a substantial positive value especially 
if there is, in the case of friction, substantial sliding. 
29.8.5  Contact Damping 
Viscous contact damping has been added to all contact options including single 
surface contact.  The original intent was to damp out oscillations normal to the contact 
surfaces  during  metal  forming  operations;  however,  it  was  later  found  to  work 
effectively  in  removing  high  frequency  noise  in  problems  which  involve  impact.    The 
input requires a damping value as a percentage of critical, 2𝑚, where 𝑚 is the mass and 
𝜔  is  the  natural  frequency.    Letting  𝑘  denote  the  interface  stiffness,  we  compute  the 
natural frequency for an interface slave node from Equation 26.15.
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
Figure 29.17.  Reaction forces with and without contact damping. 
𝜔 = √
𝑘(𝑚slave + 𝑚master)
𝑚slave𝑚master
𝑚 = min{𝑚slave, 𝑚master}.
(29.24)
The  master  mass  𝑚master  is  interpolated  from  the  master  nodes  of  the  segment 
containing the slave node using the basis functions evaluated at the contact point of the 
slave node.   
Force  oscillations  often  occur  as  curved  surfaces  undergo  relative  motion.    In 
these  cases  contact  damping  will  eliminate  the  high  frequency  content  in  the  contact 
reaction  forces  but  will  be  unable  to  damp  the  lower  frequency  oscillations  caused  by 
nodes moving from segment to segment when there is a large angle change between the 
segments.  This is shown in the hemispherical punch deep drawing in Figure 29.16.  The 
reaction  forces  with  and  without  contact  damping  in  Figure  29.17  show  only  minor 
differences  since  the  oscillations  are  not  due  to  the  dynamic  effects  of  explicit 
integration.    However,  refining  the  mesh  as  shown  in  Figure  29.18  to  include  more 
elements  around  the  die  corner  as  in  Figure  29.18  greatly  reduces  the  oscillations  as 
shown in Figure 29.19.  This shows the importance of using an adequate mesh density 
in applications where significant relative motion is expected around sharp corners.
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
Figure 29.18.  Refinement of die radius. 
  Friction  
Figure  29.19.    The  oscillations  are  effectively  eliminated  by  the  mesh 
refinement.
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
Friction  in  LS-DYNA  is  based  on  a  Coulomb  formulation.    Let  𝐟∗  be  the  trial 
force, 𝐟𝑛 the normal force, 𝑘 the interface stiffness, 𝜇 the coefficient of friction, and 𝐟𝑛 the 
frictional force at time 𝑛.  The frictional algorithm, outlined below, uses the equivalent 
of an elastic plastic spring.  The steps are as follows:  
1. Compute the yield force, 𝐹𝑦: 
𝐹𝑦 = 𝜇 |𝐟𝑛|
2. Compute the incremental movement of the slave node  
𝑛)
𝑛, 𝜂𝑐
Δ𝐞 = 𝐫𝑛+1(𝜉𝑐
𝑛+1) − 𝐫𝑛+1(𝜉𝑐
𝑛+1, 𝜂𝑐
3. Update the interface force to a trial value: 
4. Check the yield condition: 
𝐟∗ = 𝐟𝑛 − 𝑘Δ𝐞
𝐟𝑛+1 = 𝐟∗
if ∣𝐟∗∣ ≤ 𝐹𝑦
5. Scale the trial force if it is too large: 
𝐟𝑛+1 =
𝐹𝑦𝐟∗
|𝐟∗|
if ∣𝐟∗∣ > 𝐹𝑦
(29.25)
(29.26)
(29.27)
(29.28)
(29.29)
An exponential interpolation function smooths the transition between the static, 
𝜇𝑠, and dynamic, 𝜇𝑑, coefficients of friction where 𝐯 is the relative velocity between the 
slave node and the master segment: 
where 
𝜇 = 𝜇𝑑 + (𝜇𝑠 − 𝜇𝑑) 𝑒−𝑐|𝐯|,
𝐯 =
Δ𝐞
Δ𝑡
,
Δ𝑡 is the time step size, and 𝑐 is a decay constant. 
(29.30)
(29.31)
The  interface  shear  stress  that  develops  as  a  result  of  Coulomb  friction  can  be 
very  large  and  in  some  cases  may  exceed  the  ability  of  the  material  to  carry  such  a 
stress.    We  therefore  allow  another  limit  to  be  placed  on  the  value  of  the  tangential 
force:   
𝑓 𝑛+1 = min(𝑓Coulomb
𝑛+1
, 𝜅𝐴master),
(29.32)
where 𝐴master  is  the  area  of  the  master  segment  and  𝜅  is  the  viscous  coefficient.    Since 
more than one node may contribute to the shear stress of a segment, we recognize that 
the stress may still in some cases exceed the limit 𝜅. 
Typical  values  of  friction,  see  Table  26.1,  can  be  found  in  Marks  Engineering 
Handbook.
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
MATERIALS 
Hard steel on hard steel 
Mild steel on mild steel 
Aluminum on mild steel 
Aluminum on aluminum1 
Tires on pavement (40psi) 
STATIC 
0.78 (dry) 
0.74 (dry) 
0.61 (dry) 
05 (dry) 
0.90 (dry). 
SLIDING 
08 (greasy), .42 (dry) 
10 (greasy), .57 (dry) 
47 (dry) 
1.4 (dry) 
69(wet), .85(dry) 
Table 26.1.  Typical values of Coulomb Friction [Marks] 
29.9  Tied Interfaces 
Sudden transitions in zoning are permitted with the tied interfaces as shown in 
Figure 29.20  where  two  meshes  of  solid  elements  are  joined.    This  feature  can  often 
decrease the amount of effort required to generate meshes since it reduces the need to 
match nodes across interfaces of merged parts. 
Tied  interfaces  include  four  interface  options  of  which  three  are  in  the  Sliding 
Interface Definition Section in the LS-DYNA User’s Manual.  These are: 
•  Type 2 for tying surfaces with translational degrees of freedom. 
•  Type 6 for tying translational degrees of freedom of nodes to a surface 
Figure 29.20.  Tied interface used for a mesh transition. 
Tied interface permits
mesh transitions
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
•  Type 7 for tying both translational and rotational degrees of freedom of nodes 
The fourth option is in the “Tie-Breaking Shell Definitions” Section of the user’s 
manual and is meant as a way of tying edges of adjacent shells together.  Unlike Type 7 
this latter option does not require a surface definition, simply nodal lines, and includes 
a  failure  model  based  on  plastic  strain  which  can  be  turned  off  by  setting  the  plastic 
failure  strain  to  a  high  value.    The  first  two  options,  which  are  equivalent  in  function 
but  differ  in  the  input  definition,  can  be  properly  applied  to  nodes  of  elements  which 
lack rotational degrees of freedom.  The latter options must be used with element types 
that  have  rotational  degrees  of  freedom  defined  at  their  nodes  such  as  the  shell  and 
beam elements.  One important application of Type 7 is that it allows edges of shells to 
be  tied  to  shell  surfaces.    In  such  transitions  the  shell  thickness  is  not  considered.  
Exceptions  from  these  latter  statements  is  in  case  of  invoking  the  implicit  accuracy 
option,  see  *CONTROL_ACCURACY,  for  which  a  node  with  rotational  degrees  of 
freedom  can  tie  to  any  element  with  or  without  offset.    In  this  case  moments  are 
consistently transferred based on the kinematics of the chosen tied interface, the theory 
for this is presented in Section.   
Since  the  constraints  are  imposed  only  on  the  slave  nodes,  the  more  coarsely 
meshed  side  of  the  interface  is  recommended  as  the  master  surface.    Ideally,  each 
master  node  should  coincide  with  a  slave  node  to  ensure  complete  displacement 
compatibility along the interface, but in practice this is often difficult if not impossible to 
achieve.    In  other  words,  master  nodes  that  do  not  coincide  with  a  slave  node  can 
interpenetrate through the slave surface. 
Implementation  of  tied  interface  constraints  is  straightforward.    Each  time  step 
we  loop  through  the  tied  interfaces  and  update  each  one  independently.    First,  we 
distribute  the  nodal  forces  and  nodal  mass  of  each  slave  node  to  the  master  nodes 
which define the segment containing the contact point, i.e., the increments in mass and 
forces 
Δ𝑓𝑚
𝑖 = 𝜙𝑖(𝜉𝑐,𝜂𝑐)𝑓𝑠
(29.33)
are added to the mass and force vector of the master surface.  After the summation over 
all slave nodes is complete, we can compute the acceleration of the master surface.  The 
acceleration  of  each  slave  node  𝑎𝑖𝑠  is  then  interpolated  from  the  master  segment 
containing its contact points: 
𝑎𝑖𝑠 = ∑ 𝜙𝑗(𝜉𝑐, 𝜂𝑐)𝑎𝑖
.
𝑗=1
(29.34)
Velocities and displacements are now updated normally. 
The  interpolated  contact  point,  (𝜉𝑐, 𝜂𝑐),  for  each  slave  node  is  computed  once, 
since  its  relative  position  on  the  master  segment  is  constant  for  the  duration  of  the 
calculation.  If the closest point projection of the slave node to the master surface is non-
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
orthogonal, values  of (𝜉𝑐, 𝜂𝑐)  greater  than  unity  will  be  computed.    To  allow  for  slight 
errors  in  the  mesh  definition,  the  slave  node  is  left  unconstrained  if  the  magnitude  of 
the  contact  point  exceeds  1.02.    Great  care  should  be  exercised  in  setting  up  tied 
interfaces to ensure that the slave nodes are covered by master segments. 
Conflicting  constraints  must  be  avoided.    Care  should  be  taken  not  to  include 
nodes  that  are  involved  in  a  tied  interfaces  in  another  tied  interface,  in  constraint  sets 
such  as  nodal  constraint  sets,  in  linear  constraint  equations,  and  in  spot  welds.  
Furthermore,  tied  interfaces  between  rigid  and  deformable  bodies  are  not  permitted.  
LS-DYNA  checks  for  conflicting  constraints  on  nodal  points  and  if  such  conflicts  are 
found,  the  calculation  will  terminate  with  an  error  message  identifying  the  conflict.  
Nodes in tied interfaces should not be included as slave nodes in rigid wall definitions 
since  interactions  with  stonewalls  will  cause  the  constraints  that  were  applied  in  the 
tied interface logic to be violated.  We do not currently check for this latter condition is 
LS-DYNA.  
Tied interfaces require coincident surfaces and for shell element this means that 
the mid-surfaces must be coincident.  Consider Figure 29.21 where identical slave and 
master  surfaces  are  offset.    In  this  case  the  tied  constraints  require  that  translational 
velocities of tied nodes be identical, i.e., 
𝐯𝑠 = 𝐯𝑚.
(29.35)
Consequently, if the nodes are offset, rotations are not possible.  The velocity of a tied 
slave node in Figure 29.21 should account for the segment rotation: 
𝐯𝑠 = 𝐯𝑚 − 𝑧̂ 𝐞3 × 𝛚,
(29.36)
where 𝑧̂ is the distance to the slave node, 𝐞3 is the normal vector to the master surface at 
the  contact  point,  and  𝛚  is  the  angular  velocity.    Since  this  is  not  the  case  in  the  tied 
interfaces logic, 𝑧̂ must be of zero length.   
LS-DYNA  projects  tied  slave  nodes  back  to  the  master  surface  if  possible  and 
prints warning messages for all projected offset nodes or nodes too far away to tie.  This 
projection  eliminates  the  problems  with  rotational  constraints  but  creates  other 
difficulties: 
•  Geometry is modified 
•  Tied  interfaces  must  be  excluded  from  automatic  generation  since  tied  surfaces 
cannot be mixed with automatic contact with thickness offsets.
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
Slave Surface
Master Surface
Figure 29.21.  Offset tied interface. 
An  offset  capability  has  been  added  to  the  tied  interfaces  which  uses  a  penalty 
approach.    The  penalty  approach  removes  the  major  limitations  of  the  constraint 
formulation since with the offset option: 
•  Multiple tied interfaces cannot share common nodes. 
•  Rigid body nodes can be constrained. 
•  Tied interface nodes can have other constraints applied and can be subjected to 
prescribed motions. 
29.10  Strongly Objective Tied Contacts 
In  implicit  calculations,  non-physical  results  observed  when  some  tied  contact 
formulations  are  combined  with  automatic  single  point  constraints  on  solid  element 
rotational  degrees  of  freedom  (AUTOSPC  on  *CONTROL_IMPLICIT_SOLVER)  have 
motivated  an  extension  in  this  context.    A  goal  is  to  provide  a  universal  tied  contact 
formulation  in  implicit  that  works  well  in  most  situations,  thus  preventing  the  user 
from having to think too hard about which interface is best suited for the application at 
hand.    To  this  end,  a  small  selection  of  tied  interfaces  have  been  singled  out  that  all 
represent this universal contact, these are 
*CONTACT_TIED_NODES_TO_SURFACE_CONSTRAINED_OFFSET
*CONTACT_TIED_NODES_TO_SURFACE_OFFSET
*CONTACT_TIED_SHELL_EDGE_TO_SURFACE_CONSTRAINED_OFFSET 
*CONTACT_TIED_SHELL_EDGE_TO_SURFACE_BEAM_OFFSET 
The first of these two do not consider rotational degrees of freedom, whereas the other 
two  do.    Furthermore,  the  first  and  third  are  constraint  based  and  the  other  two  are 
penalty  based,  so  all  in    all  these  four  cover  much  of  what  a  user  expects  from  a  tied 
interface.    By  setting  IACC  to  1  on  *CONTROL_ACCURACY  any  of  the  tied  contact 
options  mentioned  above  (and  the  non-offset  counterparts  as  a  side  effect,  i.e., 
*CONTACT_TIED_NODES_TO_SURFACE 
and 
*CONTACT_TIED_SHELL_EDGE_TO_SURFACE)  are 
this  strongly 
objective formulation.  In addition to being strongly objective, i.e., forces and moments 
treated  with
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
transform correctly under superposed rigid body motions in a single implicit step, this 
formulation  applies  rotational  constraints  consistently  when  and  only  when  necessary. 
This  means  not  only  that  slave  nodes  without  rotational  degrees  of  freedom  are  not 
rotationally constrained, but also that bending and torsional rotations are constrained to 
the master segment’s rotational motion in a way that is physically justified.  To be more 
specific, slave node bending rotations (i.e., rotations in the plane of the master segment) 
are constrained to the master segment rotational degrees of freedom if this happens to 
stem  from  a  shell  element,  otherwise  they  are  constrained  to  the  master  segment 
rotation as determined from its individual nodal translations.  The slave node torsional 
rotations  (i.e.,  rotations  with  respect  to  the  normal  of  the  master  segment)  are  always 
constrained  according  to  this  latter  philosophy,  thus  avoiding  a torsional  constraint to 
the  relatively  weak  drilling  mode  of  shells.    So  this  tied  contact  formulation  properly 
treats  bending  and  torsional  rotations,  here  slave  node  rotational  degrees  of  freedom 
typically  come  from  shell  or  beam  elements.    So  in  effect,  it  is  in  a  sense  sufficient  to 
only consider 
*CONTACT_TIED_SHELL_EDGE_TO_SURFACE_CONSTRAINED_OFFSET 
*CONTACT_TIED_SHELL_EDGE_TO_SURFACE_BEAM_OFFSET 
for  most  situations  (choosing  between  a  constraint  or  penalty  formulation)    but  the 
other two 
*CONTACT_TIED_NODES_TO_SURFACE_CONSTRAINED_OFFSET
*CONTACT_TIED_NODES_TO_SURFACE_OFFSET 
“non-rotational”  formulations  are  included  in  the  event  of  not  wanting  to  constrain 
rotations  whatsoever.    Referring  to  Figure  2929-22,  the  following  is  the  mathematical 
formulation of this tied contact formulation.
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
𝑬0 
𝛼𝜆 
𝑭0 
𝑮0 
𝑠 
𝑝 
𝑚4 
𝜆 
𝑀 
𝑡 = 0 
𝑚2
𝑚1 
𝑬 
𝑭 
Tying 
point 
𝑚3
𝑡 > 0
Figure  2929-22  Kinematics  of  the  implicit  strong  objective  tied  contact 
formulation 
29.10.1  Kinematics 
We consider a slave node 𝑠 tied to a master segment 𝑀 with an offset 𝜆, the slave node 
projection  onto  the  master  segment  is  denoted  𝑝.  Let  𝒙𝑠  denote  the  slave  node 
coordinate and 
𝒙𝑝 = ∑ ℎ𝑖𝒙𝑚
𝑖=1
(29.37)
be  the  slave  node  projection  on  the  master  segment,  where  ℎ𝑖  are  the  constant 
isoparametric  weights.    To  each  of  𝑠,  𝑝  and    𝑀  we  associate  orthonormal  bases 
(coordinate systems) represented by 
𝑬 = {𝒆1
𝒆2
𝒆3}
𝑭 = {𝒇1
𝒇2
𝒇3} 
(29.38)
(29.39)
𝒈2
𝒈3},
𝑮 = {𝒈1
(29.40)
respectively.    The  orthogonal  matrix  𝑮  is  the  master  segment  coordinate  system 
𝑖   with  normal  𝒈3.  At  𝑡 = 0,  we 
expressed  as  a  function  of  the  master  coordinates  𝒙𝑚
initialize  𝑬0 = 𝑭0 = 𝑮0  but  𝑬  and  𝑭  then  evolves  independently  based  on  the  nodal 
rotational velocities 𝝎𝑠 and 
In  the  numerical  implementation,  if  ∆𝜽𝑠 = 𝝎𝑠∆𝑡  and  ∆𝜽𝑝 = 𝝎𝑝∆𝑡  are  the  incremental 
rotations of s and p at a given time step, then the coordinate systems are updated 
𝝎𝑝 = ∑ ℎ𝑖𝝎𝑚
𝑖=1
. 
(29.41)
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
𝑬𝑛+1 = 𝑹(∆𝜽𝑠)𝑬𝑛
(29.42)
𝑭𝑛+1 = 𝑹(∆𝜽𝑝)𝑭𝑛 
(29.43)
where  𝑹(∆𝜽)  denotes  the  finite  rotation  matrix  corresponding  to  the  rotational 
increment ∆𝜽. Of course, this only makes sense if the slave node and/or master segment 
have  rotational  degrees  of  freedom.    If  the  slave  node  lacks  rotational  degrees  of 
freedom, then neither bending nor torsion is constrained and 𝑬 is of no interest.  If on 
the other hand the master segment lacks rotational degrees of freedom, then we use 𝑭 =
𝑮 which is still of interest to deal with the offset, 𝑮 is always well-defined.  LS-DYNA 
automatically detects rotational degrees of freedom and takes the proper measures. 
29.10.2  Translational constraint 
Given the notation in the previous section and referring to Figure 2929-22,  
𝒅 = {𝒙𝑠 − 𝛼𝜆𝒆3} − {𝒙𝑝 + (1 − 𝛼)𝜆𝒇3} 
(29.44)
represents the vector we want to be zero in the translational part of the contact.  Here 𝜆 
is  the  offset  distance  between  𝑝  and  𝑠  and  is  constant  throughout  the  simulation.  
Furthermore,  𝛼  is  a  constant  between  0  and  1  that  determines  the  actual  tying  point 
according to the following simple rules.  First, if the slave node is connected to a solid or 
beam  element  or  if  the  contact  definition  does  not  take  rotational  degrees  of  freedom 
into account, then 𝛼 = 0. Otherwise, if the slave node is connected to a shell element and 
the  master  segment  is  connected  to  a  solid  element,  then  𝛼 = 1.  If  neither  of  those 
situations  apply  then  both  slave  and  master  sides  must  connect  to  shell  elements,  for 
which 𝛼 = 0.5, so note that the value of 𝛼 is not accounting for the relative difference in 
shell thicknesses but assumes equal shell thickness on both master and slave sides.  For 
and 
*CONTACT_TIED_NODES_TO_SURFACE_CONSTRAINED_OFFSET 
*CONTACT_TIED_SHELL_EDGE_TO_SURFACE_CONSTRAINED_OFFSET, 
this 
condition is imposed as a constraint 
for 
(29.45)
and 
whereas 
*CONTACT_TIED_SHELL_EDGE_TO_SURFACE_BEAM_OFFSET 
penalty 
formulation  is  used.    To  this  end  we  use  a  constitutive  relation  between  force  and 
displacement 
*CONTACT_TIED_NODES_TO_SURFACE_OFFSET 
𝒅 = 𝟎
a 
(29.46)
with  𝐾𝑓   as  the  penalty  stiffness.    Then  an  energy  principle  is  employed  to  identify  the 
nodal forces and moments, 
𝒇 = 𝐾𝑓 𝒅
𝑇𝛿𝑿, 
(29.47)
where  𝑿  is  nodal  coordinate  array  of  the  slave  master  pair,  and  𝛿  is  the  variation 
operator.  Identifying 𝑩𝑓  by 
𝒇 𝑇𝛿𝒅 = 𝑷𝑓
𝛿𝒅 = 𝑩𝑓 𝛿𝑿
(29.48)
the nodal force array is given by 
𝑇𝒇 . 
(29.49)
Worth noticing is that 𝑩𝑓  is the constraint matrix corresponding to the constraint variant 
of the contact. 
𝑷𝑓 = 𝑩𝑓
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
29.10.3  Bending and torsion constraint 
If the slave node has rotational degrees of freedom and the contact formulation is said 
to treat those, bending and torsion is constrained.  The bending strain is calculated as 
(29.50)
which essentially is a measure of the amount 𝒆3 and 𝒇3 deviates from being parallel.  The 
torsional strain is a scalar given by  
𝜑𝑗 = 𝒈𝑗
𝑗 = 1,2 
𝑇(𝒆3 × 𝒇3),
𝑇𝒈2 − 𝒆2
and is a measure of the relative rotation between 𝑬 and 𝑮 with respect to the normal 𝒈3. 
The constraint to enforce is  
𝑇𝒈1) 
𝜑3 =
(29.51)
(𝒆1
𝝋 =
⎜⎛
⎝
𝜑1
𝜑2
𝜑3⎠
⎟⎞ = 𝟎 
(29.52)
which  for  a  penalty  formulation  leads  to  a  constitutive  relation  between  moment  and 
rotation vector 
(29.53)
with  𝐾𝑚  being  a  stiffness  parameter.    Following  the  approach  for  translational 
treatment, we get the nodal force contribution 
𝑇 𝒎
𝒎 = 𝐾𝑚𝝋
(29.54)
𝑷𝑚 = 𝑩𝑚
where 
Also here 𝑩𝑚 is the constraint matrix in case a constraint formulation is used. 
𝛿𝝋 = 𝑩𝑚𝛿𝑿.
(29.55)
The  formulae  for  𝐾𝑓   and  𝐾𝑚  are  found  in  earlier  sections  on  tied  interfaces  while  the 
expressions for the matrices 𝑩𝑓  and  𝑩𝑚 are quite involved and omitted for the sake of 
clarity, the nodal forces and moments are implemented by using (manual) algorithmic 
differentiation. 
29.11  Sliding-Only Interfaces 
This option is seldom useful in structural calculations.  Its chief usefulness is for treating 
interfaces  where  the  gaseous  detonation  products  of  a  high  explosive  act  on  a  solid 
material.    The  present  algorithm,  though  simple,  has  performed  satisfactorily  on  a 
number of problems of this latter type.  We briefly outline the approach here since the 
algorithm is still experimental and subject to change. 
The method consists of five steps.  In the first step, the mass per unit area (mass/area) 
and  pressure  are  found  at  each  node  on  the  slave  surface.    Next,  the  contact  point  for 
each master node is found, and the slave mass/area and slave pressure at each master 
node is interpolated from the slave surface.  In the third step, this pressure distribution 
is applied to the master surface to update its acceleration.  In the fourth step, the normal 
component  of  the  acceleration  at  each  node  on  the  master  surface  is  scaled  by  its  z-
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
tied interface
Figure 29.23.  Incremental searching may fail on surfaces that are not simply
connected.    The  new  contact  algorithm  in  LS-DYNA  avoids  incremental 
searching  for  nodal  points  that  are  not  in  contact  and  all  these  cases  are
considered. 
factor defined as the mass/area of the master surface at the master node divided by the 
sum of the mass/area of the slave surface at the master node.  The last step consists of 
resetting the normal acceleration and velocity components of all slave nodes to ensure 
compatibility. 
29.12  Bucket Sorting 
Bucket sorting is now used extensively in both the surface to surface and single surface 
contact  algorithms.    Version  920  of  LS-DYNA  no  longer  contains  one-dimensional 
sorting.    Presently  two  separate  but  similar  bucket  sorts  are  in  LS-DYNA.    In  the  first 
and  older  method  we  attempt  to  find  for  each  node  the  three  nearest  nodes.    In  the 
newer method which is systematically replacing the older method we locate the nearest 
segment. 
The reasons for eliminating slave node tracking by incremental searching is illustrated 
in Figure 29.23 where surfaces are shown which cause the incremental searches to fail.  
In LS-DYNA tied interfaces are used extensively in many models creating what appears 
to the contact algorithms to be topologically disjoint regions.  For robustness, our new 
algorithms  account  for  such  mesh  transitions  with  only  minor  cost  penalties.    With 
bucket  sorting  incremental  searches  may  still  be  used  but  for  reliability  they  are  used
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
Bucket
Y Strips
Figure 29.24.  One- and two-dimensional bucket sorting. 
after  contact  is  achieved.    As  contact  is  lost,  the  bucket  sorting  for  the  affected  nodal 
points must resume. 
In  a  direct  search  of  a  set  of  𝑁  nodes  to  determine  the  nearest  node,  the  number  of 
distance  comparisons  required  is  𝑁 − 1.    Since  this  comparison  needs  to  be  made  for 
each node, the total number of comparisons is 𝑁(𝑁 − 1), with each of these comparisons 
requiring a distance calculation 
12 = (𝑥𝑖 − 𝑥𝑗)2 + (𝑦𝑖 − 𝑦𝑗)2 + (𝑧𝑖 − 𝑧𝑗)2,
(29.56)
that  uses  eight  mathematical  operations.    The  cumulative  effect  of  these  mathematical 
operations  for  𝑁(𝑁 − 1)  compares  can  dominate  the  solution  cost  at  less  than  100 
elements. 
The idea behind a bucket sort is to perform some grouping of the nodes so that the sort 
operation need only calculate the distance of the nodes in the nearest groups.  Consider 
the  partitioning  of  the  one-dimensional  domain  shown  in  Figure  29.24.    With  this 
partitioning the nearest node will either reside in the same bucket or in one of the two 
adjoining buckets.  The number of distance calculations is now given by
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
3𝑁
− 1,
(29.57)
where  𝑎  is  the  number  of  buckets.    The  total  number  of  distance  comparisons  for  the 
entire one-dimensional surface is 
𝑁 (
3𝑁
− 1).
(29.58)
Thus, if the number of buckets is greater than 3, then the bucket sort will require fewer 
distance  comparisons  than  a  direct  sort.    It  is  easy  to  show  that  the  corresponding 
number  of  distance  comparisons  for  two-dimensional  and  three-dimensional  bucket 
sorts are given by 
𝑁 (
9𝑁
𝑎𝑏
𝑁 (
27𝑁
𝑎𝑏𝑐
− 1) for 2D
− 1) for 3D
(29.59)
(29.60)
where 𝑏 and 𝑐 are the number of partitions along the additional dimension. 
The  cost  of  the  grouping  operations,  needed  to  form  the  buckets,  is  nearly  linear  with 
the  number  of  nodes  𝑁.    For  typical  LS-DYNA  applications,  the  bucket  sort  is  100  to 
1000  times  faster  than  the  corresponding  direct  sort.    However,  the  sort  is  still  an 
expensive part of the contact algorithm, so that, to further minimize this cost, the sort is 
performed every ten or fifteen cycles and the nearest three nodes are stored.  Typically, 
three  to  five  percent  of  the  calculational  costs  will  be  absorbed  in  the  bucket  sorting 
when most surface segments are included in the contact definition. 
29.12.1  Bucket Sorting in TYPE 4 Single Surface Contact 
We  set  the  number  of  buckets  in  the  𝑥,  𝑦,  and  𝑧  coordinate  directions  to 𝑁𝑋,  𝑁𝑌,  and 
𝑁𝑍,  respectively.    Letting  LMAX  represent  the  longest  characteristic  length  (found  by 
checking  the  length  of  the  segment  diagonals  and  taking  a  fraction  thereof)  over  all 
segments in the contact definition, the number of buckets in each direction is given by 
𝑥max − 𝑥min
LMAX
𝑁𝑋 =
(29.61)
,
𝑁𝑌 =
𝑦max − 𝑦min
LMAX
,
(29.62)
𝑧max − 𝑧min
LMAX
where the coordinate pairs (𝑥min, 𝑥max), (𝑦min, 𝑦max), and (𝑧min, 𝑧max) define the extent 
of the contact surface and are updated each time the bucket searching is performed.  In 
order  to  dynamically  allocate  memory  effectively  with  FORTRAN,  we  further  restrict 
𝑁𝑍 =
(29.63)
,
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
the  number  of  buckets  such  that  the  total  number  of  buckets  does  not  exceed  the 
number of nodes in the contact surface, NSN or 5000: 
𝑁𝑋 ⋅ 𝑁𝑌 ⋅ 𝑁𝑍 ≤ MIN (NSN, 5000).
(29.64)
If  the  characteristic  length, LMAX,  is  large  due  to  an  oversized  contact  segment  or  an 
instability  leading  to  a  node  flying  off  into  space,  the  bucket  sorting  can  be  slowed 
down  considerably  since  the  number  of  buckets  will  be  reduced.    In  older  versions  of 
DYNA3D this led to the error termination message “More than 1000 nodes in bucket.” 
The formulas given by Belytschko and Lin [1985] are used to find the bucket containing 
a node with coordinates (𝑥, 𝑦, 𝑧).  The bucket pointers are given by 
𝑃𝑋 = 𝑁𝑋 ⋅
(𝑥 − 𝑥min)
(xmax − xmin)
+ 1,
PY = NY ⋅
(𝑦 − 𝑦min)
(𝑦max − 𝑦min)
+ 1,
PZ = NZ ⋅
(𝑧 − 𝑧min)
(𝑧max − 𝑧min)
+ 1,
and are used to compute the bucket number given by 
NB = PX + (PY − 1) ⋅ PX + (PZ − 1) ⋅ PX ⋅ PY.
(29.65)
(29.66)
(29.67)
(29.68)
For  each  nodal  point, 𝑘,  in  the  contact  surface  we  locate  the  three nearest  neighboring 
nodes by searching all nodes in buckets from 
MAX(1, PX1), MIN(NX, PX + 1),
MAX(1, PY1), MIN(NY, PY + 1),
MAX(1, PZ1), MIN(NZ, PZ + 1).
(29.69)
(29.70)
(29.71)
A maximum of twenty-seven buckets are searched.  Nodes that share a contact segment 
with k are not considered in this nodal search.  By storing the three nearest nodes and 
rechecking  these  stored  nodes  every  cycle  to  see  if  the  nearest  node  has  changed,  we 
avoid performing the bucket sorting every cycle.  Typically, sorting every five to fifteen 
cycles is adequate.  Implicit in this approach is the assumption that a node will contact 
just one surface.  For this reason the single surface contact (TYPE 4 in LS-DYNA) is not 
applicable to all problems.  For example, in metal forming applications both surfaces of 
the workpiece are often in contact. 
The  nearest  contact  segment  to  a  given  node,  𝑘,  is  defined  to  be  the  first  segment 
encountered when moving in a direction normal to the surface away from 𝑘.  A major 
deficiency  with  the  nearest  node  search  is  depicted  in  Figure  29.25  where  the  nearest 
nodes are not even members of the nearest contact segment.  Obviously, this would not
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
be  a  problem  for  a  more  uniform  mesh.    To  overcome  this  problem  we  have  adopted 
segment based searching in both surface to surface and single surface contact. 
29.12.2  Bucket Sorting in Surface to Surface and TYPE 13 Single Surface Contact 
The procedure is roughly the same as before except we no longer base the bucket size 
on  𝐿𝑀𝐴𝑋  which  can  result  in  as  few  as  one  bucket  being  generated.    Rather,  the 
product  of  the  number  of  buckets  in  each  direction  always  approaches  𝑁𝑆𝑁  or  5000 
whichever is smaller,  
NX ⋅ NY ⋅ NZ ≤ MIN(NSN, 5000),
(29.72)
where  the  coordinate  pairs  (𝑥min, 𝑥max),  (𝑦min, 𝑦max),  and  (𝑧min, 𝑧max)  span  the  entire 
contact surface.  In the new procedure we loop over the segments rather than the nodal 
points.    For  each  segment  we  use  a  nested  DO  LOOP  to  loop  through  a  subset  of 
buckets from IMIN to IMAX, JMIN to JMAX, and to KMAX where 
IMIN = MIN(PX1, PX2, PX3, PX4),
IMAX = MAX(PX1, PX2, PX3, PX4),
JMIN = MIN(PY1, PY2, PY3, PY4),
KMIN = MIN(PZ1, PZ2, PZ3, PZ4),
KMAX = MAX(PZ1, PZ2, PZ3, PZ4),
(29.73)
(29.74)
(29.75)
(29.76)
(29.77)
and  PX𝑘,  PY𝑘,  PZ𝑘  are  the  bucket  pointers  for  the  kth  node.    Figure  29.26  shows  a 
segment passing through a volume that has been partitioned into buckets.   
We  check  the  orthogonal  distance  of  all  nodes  in  the  bucket  subset  from  the  segment.  
As  each  segment  is  processed,  the  minimum  distance  to  a  segment  is  determined  for 
every  node  in  the  surface  and  the  two  nearest  segments  are  stored.    Therefore  the 
required storage allocation is still deterministic.  This would not be the case if we stored 
Normal vector at
node 3
Figure  29.25.    Nodes  2  and  4  share  segments  with  node  3  and  therefore  the
two nearest nodes are1 and 5.  The nearest contact segment is not considered
since its nodes are not members of the nearest node set.
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
Nodes in buckets shown are checked for
contact with the segment
Figure 29.26.  The orthogonal distance of each slave node contained in the box
from the segment is determined.  The box is subdivided into sixty buckets. 
for each segment a list of nodes that could possibly contact the segment. 
We  have  now  determined  for  each  node,  𝑘,  in  the  contact  surface  the  two  nearest 
segments for contact.  Having located these segments we permanently store the node on 
these segments which  is nearest to node 𝑘.  When checking for interpenetrating nodes 
we  check  the  segments  surrounding  the  node  including  the  nearest  segment  since 
during  the  steps  between  bucket  searches  it  is  likely  that  the  nearest  segment  may 
change.    It  is  possible  to  bypass  nodes  that  are  already  in  contact  and  save  some 
computer  time;  however,  if  multiple  contacts  per  node  are  admissible  then  bypassing 
the search may lead to unacceptable errors. 
29.13  Single Surface Contact Algorithms in LS-DYNA 
The  single  surface  contact  algorithms  evolved  from  the  surface  to  surface  contact 
algorithms  and  the  post  contact  searching  follows  the  procedures  employed  for  the 
surface to surface contact.  Type 4 contact in LS-DYNA uses the following steps where 
NSEG  is  the  number  of  contact  segments  and  NSN  is  the  number  of  nodes  in  the 
interface:  
•  Loop through the contact segments from 1 to NSEG 
◦  Compute  the  normal  segment  vectors  and  accumulate  an  area  weighted 
average  at  the  nodal  points  to  determine  the  normal  vectors  at  the  nodal 
points.
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
•  Loop through the slave nodes from 1 to NSN 
◦  Check  all  nearest  nodes,  stored  from the  bucket  sort,  and  locate  the  node 
which is nearest. 
◦  Check  to  see  if  nearest  node  is  within  a  penetration  tolerance  determined 
during the bucket sort, if not, proceed to the end of the loop. 
◦  For  shell  elements,  determine  if  the  nearest  node  is  approaching  the  seg-
ment from the positive or negative side based on the right hand rule.  Pro-
ject both the node and the contact segment along the nodal normal vectors 
to account for the shell thickness.   
◦  Check  for  interpenetrating  nodes  and  if  a  node  has  penetrated  apply  a 
nodal point force that is proportional to the penetration depth. 
End of Loop 
Of  course,  several  obvious  limitations  of  the  above  procedure  exists.    The  normal 
vectors that are used to project the contact surface are meaningless for nodes along an 
intersection of two or more shell surfaces (Please see the sketch at the bottom of Figure 
29.27).      In  this  case  the  normal  vector  will  be  arbitrarily  skewed  depending  on  the 
choice  of  the  numbering  of  the  connectivities  of  the  shells  in  the  intersecting  surfaces.  
Secondly,  by  considering  the  possibility  of  just  one  contact  segment  per  node,  metal 
forming  problems  cannot  be  handled  within  one  contact  definition.    For  example,  if  a 
workpiece  is  constrained  between  a  die  and  a  blankholder  then  at  least  some  nodal 
points in the workpiece must necessarily be in contact with two segments-one in the die 
and  the  other  in  the  workpiece.    These  two  important  limitations  have  motivated  the 
development  of  the  new  bucket  sorting  procedure  described  above  and  the  modified 
single surface contact procedure, type 13.  
A  major  change  in  type  13  contact  from  type  4  is  the  elimination  of  the  normal  nodal 
vector projection by using the segment normal vector as shown in Figure 29.27.   
Segment numbering within the contact surface is arbitrary when the segment normal is 
used greatly simplifying the model input generation.  However, additional complexity 
is  introduced  since  special  handling  of  the  nodal  points  is  required  at  segment 
intersections where nodes may approach undetected as depicted in Figure 29.28a.   
To  overcome  this  limitation  an  additional  logic  that  put  cylindrical  cap  at  segment 
intersections has been introduced in contact type 13 (and a3).  See Figure 29.28b.    
Assuming the segment based bucket sort has been completed and closest segments are 
known  for  all  slave  nodes    then  the  procedure  for  processing  the  type  13  contact 
simplifies to: 
•  Loop through the slave nodes from 1 to NSN
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
Type 4
Contact surface is based
on a nodal point normal
vector projection
Type 13
Contact surface is based
on segment normal 
projection
Figure  29.27.    Projection  of  the  contact  surface  for  a  node  approaching  from 
above is shown for types 4 and 13 contact. 
◦  If node is in contact, check to see if the contact segment has changed and if 
so,  then  update  the  closest  segment  information  and  the  orientation  flag 
which remembers the side in contact.  Since no segment orientation infor-
mation is stored this flag may change as the node moves from segment to 
segment.   
◦  Check  the  closest  segment  to  see  if  the  node  is  in  contact  if  not  then  pro-
ceed to the end of the loop.  If the slave node or contact segment connectiv-
ity  is  a  member  of  a  shell  element,  project  both  the  node  and  the  contact 
segment  along  the  segment  normal  vector  to  account  for  the  shell  thick-
ness.  A nodal thickness is stored for each node and a segment thickness is 
stored for each segment.  A zero thickness is stored for solid elements.  The 
thickness can be optionally updated to account for membrane thinning. 
◦  Check  for  interpenetrating  nodes  and  if  a  node  has  penetrated  apply  a 
nodal point force that is proportional to the penetration depth. 
End of Loop 
Note that type 13 contact does not require the calculation of nodal normal vectors. 
29.14  Surface to Surface Constraint Algorithm 
The constraint algorithm that we implemented is based on the algorithm developed by 
Taylor  and  Flanagan  [1989].    This  involves  a  two-pass  symmetric  approach  with  a 
partitioning  parameter, 𝛽,  that  is  set  between negative  and  positive unity  where 𝛽 = 1
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
Figure 29.28.     
and 𝛽 = −1 correspond to one way treatments with the master surface accumulating the 
mass  and  forces  from  the  slave  surface  (for  𝛽 = 1)  and  visa  versa  (for  𝛽 = −1).    The 
searching  algorithms  are  those  used  in  the  other  contact  algorithms  for  the  surface  to 
surface contact. 
In  this  constraint  approach  the  accelerations,  velocities,  and  displacements  are  first 
updated to a trial configuration without accounting for interface interactions.  After the 
update,  a  penetration  force  is  computed  for  the  slave  node  as  a  function  of  the 
penetration distance Δ𝐿: 
𝐟𝑝 =
𝑚𝑠Δ𝐿
Δ𝑡2 𝐧,
(29.78)
where 𝐧 is the normal vector to the master surface. 
We  desire  that  the  response  of  the  normal  component  of  the  slave  node  acceleration 
vector, 𝐚s, of a slave node residing on master segment 𝑘 be consistent with the motion of 
the master segment at its contact segment (𝑠c, 𝑡c), i.e.,  
as = 𝜙1(𝑠c, 𝑡c)𝑎𝑛𝑘
1 + 𝜙2(𝑠c, 𝑡c)𝑎𝑛𝑘
2 + 𝜙3(𝑠c, 𝑡c)𝑎𝑛𝑘
3 + 𝜙4(𝑠c, 𝑡c)𝑎𝑛𝑘
4 . 
(29.79)
For  each  slave  node  in  contact  with  and  penetrating  through  the  master  surface  in  its 
trial configuration, its nodal mass and its penetration force given by Equation (29.72) is 
accumulated to a global master surface mass and force vector: 
where 
(𝑚𝑘 + ∑ 𝑚𝑘𝑠
) 𝐚𝑛𝑘 = ∑ 𝐟𝑘𝑠
,
𝑚𝑘𝑠 = 𝜙𝑘𝑚𝑠,
𝐟𝑘𝑠 = 𝜙𝑘𝐟𝑠.
(29.80)
(29.81)
(29.82)
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
After  solving  Equation  (29.78)  for  the  acceleration  vector,  𝐚nk,  we  can  obtain  the 
acceleration correction for the slave node as  
𝐚ns = 𝐚s −
𝐟p
𝑚s
.
(29.83)
The  above  process  is  repeated  after  reversing  the  master  and  slave  definitions.    In  the 
final step the averaged final correction to the acceleration vector is found 
final =
𝐚𝑛
(1 − 𝛽)𝐚𝑛
1st  pass +
(1 + 𝛽)𝐚𝑛
2nd  pass,
and used to compute the final acceleration at time 𝑛 + 1 
𝐚𝑛+1 = 𝐚trial + 𝐚𝑛
final,
(29.84)
(29.85)
Friction, as described by Taylor and Flanagan [1989], is included in our implementation.  
Friction  resists  the  relative  tangential  velocity  of  the  slave  node  with  respect  to  the 
master surface.  This relative velocity if found by subtracting from the relative velocity: 
𝐯r = 𝐯s − (𝜙1𝐯𝑘
1 + 𝜙2𝐯𝑘
2 + 𝜙3𝐯𝑘
3 + 𝜙4𝐯𝑘
4),
the velocity component normal to the master segment: 
𝐯t = 𝐯r − (𝐧 ⋅ 𝐯r)𝐧.
A trial tangential force is computed that will cancel the tangential velocity 
𝐟∗ =
𝑚𝑠𝜐𝑡
Δ𝑡
,
where υt is the magnitude of the tangential velocity vector 
𝜐𝑡 = √𝐯𝑡 ⋅ 𝐯𝑡.
(29.86)
(29.87)
(29.88)
(29.89)
The magnitude of the tangential force is limited by the magnitude of the product of the 
Coulomb friction constant with the normal force defined as 
The limiting force is, therefore, 
And 
fn = ms𝐚ns ⋅ 𝐧,
Fy = m|𝐟n|,
𝐟𝑛+1 = 𝐟∗ if
𝐟𝑛+1 =
𝐹𝑦𝐟∗
|𝐟∗|
∣𝐟∗∣ = 𝐹𝑦, 
if ∣𝐟∗∣ > 𝐹𝑦. 
(29.90)
(29.91)
(29.92)
(29.93)
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
Therefore,  using  the  above  equations  the  modification  to  the  tangential  acceleration 
component of the slave node is given by 
𝐚t = min (𝜇𝐚nt ⋅ 𝐧,
∣𝐯s∣
Δ𝑡
),
which must act in the direction of the tangential vector defined as 
𝐧t =
𝐯t
υt
.
The corrections to both the slave and master node acceleration components are: 
ats = at𝐧t,
(29.94)
(29.95)
(29.96)
asms
mk
The above process is again repeated after reversing the master and slave definitions.  In 
the final step the averaged final correction to the acceleration vector is found 
𝐚tk = −𝜙k
(29.97)
𝐧t,
final =
𝐚t
(1 − 𝛽)𝐚t
1st  pass +
(1 + 𝛽)𝐚t
2nd  pass,
and is used to compute the final acceleration at time 𝑛 + 1 
𝐚𝑛+1 = 𝐚trial + 𝐚𝑛
final + 𝐚t
final.
(29.98)
(29.99)
A  significant  disadvantage  of  the  constraint  method  relative  to  the  penalty  method 
appears  if  an  interface  node  is  subjected  to  additional  constraints  such  as  spot  welds, 
constraint  equations,  tied  interfaces,  and  rigid  bodies.    Rigid  bodies  can  often  be  used 
with  this  contact  algorithm  if  their  motions  are  prescribed  as  is  the  case  in  metal 
forming.  For the more general cases involving rigid bodies, the above equations are not 
directly  applicable  since  the  local  nodal  masses  of  rigid  body  nodes  are  usually 
meaningless.  Subjecting the two sides of a shell surface to this constraint algorithm will 
also  lead  to  erroneous  results  since  an  interface  node  cannot  be  constrained  to  move 
simultaneously on two mutually independent surfaces.  In the latter case the constraint 
technique could be used on one side and the penalty method on the other.   
The biggest advantage of the constraint algorithm is that interface nodes remain on or 
very close to the surfaces they are in contact with.  Furthermore, elastic vibrations that 
can  occur  in  penalty  formulations  are  insignificant  with  the  constraint  technique.    The 
problem related to finding good penalty constants for the contact are totally avoided by 
the latter approach.  Having both methods available is possibly the best option of all.
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
29.15  Planar Rigid Boundaries 
The  rigid  boundary  represents  the  simplest  contact  problem  and  is  therefore  treated 
separately.  As shown in Figure 29.29 the boundary is flat, finite or infinite in extent and 
is defined by an outward normal unit vector n with the origin of n at a corner point on 
the  wall  if  the  wall  is  finite  or  at  an  arbitrary  point  on  the  wall  if  the  wall  extends  to 
infinity.  The finite wall is rectangular with edges of length L and M.  Unit vectors l and 
m  lie  along  these  edges.    A  subset  of  nodes is  defined,  usually  boundary  nodes of  the 
calculational  model,  that  are  not  allowed  to  penetrate.    Let  k  represent  one  such 
n+1 be the position vector from the origin of n to k after locally 
boundary node and let rk
updating the coordinates.  Each time step prior to globally updating the velocities and 
accelerations we check k to ensure that the nodes lies within the wall by checking that 
both inequalities are satisfied: 
𝑛+1 ⋅ 𝐥 ≤ 𝐿,
𝐫𝑘
𝑛+1 ⋅ 𝐦 ≤ 𝑀.
𝐫𝑘
(29.100)
This test is skipped for the infinite rigid wall.  Assuming that the inequality is satisfied, 
we then check the penetration condition to see if k is penetrating through the wall, 
𝑛+1 ⋅ 𝐧 < 0,
𝐫𝑘
(29.101)
and if so, the velocity and acceleration components normal to the wall are set to zero: 
𝑛 − (𝐚𝑘old
𝑛 − (𝐯𝑘old
𝑛 = 𝐚𝑘old
𝐚𝑘new
𝑛 = 𝐯𝑘old
𝐯𝑘new
⋅ 𝐧)𝐧,
⋅ 𝐧)𝐧.
(29.102)
Here  𝐚𝑘  and  𝐯𝑘  are  the  nodal  acceleration  and  velocity  of  node  k,  respectively.    This 
procedure  for  stopping  nodes  represents  a  perfectly  plastic  impact  resulting  in  an 
irreversible  energy  loss.    The  total  energy  dissipated  is  found  by  taking  the  difference 
between  the  total  kinetic  energy of  all  the  nodal  points  slaved  to  the  rigid  wall  before 
and after impact with the wall.  This energy is computed and accumulated in LS-DYNA 
and is printed in the GLSTAT (global statistics) file. 
The  tangential  motion  of  the  boundary  node  may  be  unconstrained,  fully  constrained, 
or subjected to Coulomb friction while it is in contact with the rigid boundary.
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
Origin, if extent of stonewall is finite
Figure 29.29.  Vector n is normal to the stonewall.  An optional vector l can be 
defined such that 𝐦 = 𝐧 × 𝟏.  The extent of the stonewall is limited by defining
L and M.  A zero value for either of these lengths indicates that the stonewall is 
infinite in that direction. 
Coulomb friction acts along a vector defined as: 
𝐧𝑡 =
𝐯𝑘new
 𝑛
√𝐯𝑘new
 𝑛
⋅ 𝐯𝑘new
, 
(29.103)
The magnitude of the tangential force which is applied to oppose the motion is given as 
𝑓𝑡 = min
⎜⎜⎜⎛𝑚𝑠√𝐯𝑘new
Δ𝑡
⎝
⋅ 𝐯𝑘new
, 𝜇|𝐟𝑛|
, 
⎟⎟⎟⎞
⎠
(29.104)
i.e., the maximum value required to hold the node in the same relative position on the 
stonewall or the product of the coefficient of friction and the magnitude of the normal 
force whichever is less.  In Equation (29.104), ms is the mass of the slave node and f𝑛 is 
the normal force. 
29.16  Geometric Rigid Boundaries 
The  numerical  treatment  of  geometric  rigid  walls  is  somewhat  similar  to  that  for  the 
finite  planar  rigid  walls.    The  geometric  rigid  walls  can  be  subjected  to  a  prescribed 
translational motion along an arbitrarily oriented vector; however, rotational motion is 
not  permitted.    As  the  geometric  surface  moves  and  contacts  the  structure,  external 
work  is  generated  which  is  integrated  and  added  to  the  overall  energy  balance.    In 
addition to the external work, plastic work also is generated as nodes contact the wall
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
regular prism
cylinder
flat surface
sphere
Figure  29.30.    Vector  n  determines  the  orientation  of  the  generalized
stonewalls.    For  the  prescribed  motion  options  the  wall  can  be  moved  in  the
direction V as shown. 
and  assume  the  walls  normal  velocity  at  the  point  of  contact.    Contact  can  occur  with 
any  of  the  surfaces  which  enclose  the  volume.    Currently  four  geometric  shapes  are 
available including the rectangular prism, the cylinder, flat surface, and sphere.  These 
are shown in Figure 29.30. 
29.17  VDA/IGES Contact 
This  cabability allows  the user to read VDA/IGES surfaces directly into LS-DYNA for 
analysis  as  contact  surfaces.    No  mesh  generation  is  required,  and  the  contact  is 
performed against the analytic surface.  LS-DYNA supports the VDA standard and an 
important subset of the IGES entities including: 
•#100 Circle arc 
•#102 Composite Curve 
•#106 Copious data 
•#110 Lines 
•#112 Parametric polynomial curve 
•#114 Parametric polynomial surface
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
•#116 Points 
•#126 NURBS Curves 
•#128 NURBS Surfaces 
•#142 Curve on Parametric Surface 
•#144 Trimmed Parametric Surfaces 
•#402 form 7-group 
•#406 form 15-associate name 
First,  the  user  must  specify  which  VDA/IGES  surfaces,  faces,  and  groups  should  be 
attached  to  each  material.    This  is  done  primarily  through  a  special  input  file.    Faces, 
surfaces, and groups from several different VDA/IGES input files can be combined into 
groups  that  later  can  be  refered  to  by  a  user  specified  alias.    For  example,  suppose  a 
simple sheetmetal forming problem is going to be run.  The user might have an input 
file that looks like this: 
file punch.vda punch.bin { 
  alias punch { grp001 } 
} 
file die.vda die.bin { 
  alias part1 { fce001 sur002 } 
  alias part2 { fce003 } 
} 
file die2.vda die2.bin { 
  alias part3 { fce004 } 
} 
file holder.vda holder.bin { 
  alias holder { sur001 sur002 } 
} 
alias die { part1 part2 part3 } 
end 
In  this  example,  the  user  has  specified  that  the  punch  will  be  made  up  of  the  group 
"grp001"  from  the  file  "punch.vda".    The  VDA  file  is  converted  to  a  binary  file 
"punch.bin".  If this simulation is ever rerun, the VDA input can be read directly from 
the  binary  file  thereby  significantly  reducing  startup  time.    The  die  in  this  example  is 
made up of several surfaces and faces from 2 different VDA files.  This format of input 
allows the user to combine any number of faces, surfaces, and groups from any number 
of VDA files to define a single part.  This single part name is then referenced within the 
LS-DYNA input file. 
The contact algorithm works as follows.  For the sake of simplicity, we will refer to one 
point  as  being  slaved  to  a  single  part.    Again,  this  part  will  in  general  be  made  up  of 
several VDA surfaces and faces.  First, the distance from the point to each VDA surface 
is  computed  and  stored.    For  that  surface  which  is  nearest  the  point,  several  other 
parameters are stored such as the surface coordinates of the near point on the surface.
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
slave point
(x, y, z)
Figure  29.31.    The  geometry  of  the  patch  is  a  function  of  the  parametric
coordinates 𝑠 and 𝑡. 
Each  time  step  of  the  calculation  this  information  is  updated.    For  the  nearest  surface 
the new near point is calculated.  For all other surfaces the distance the point moves is 
subtracted from the distance to the surface.  This continually gives a lower bound on the 
actual distance to each VDA surface.  When this lower bound drops below the thickness 
of the point being tracked, the actual distance to the surface is recalculated.  Actually, if 
the nearest surface is further away from the point than some distance, the near point on 
the  surface  is  not  tracked  at  all  until  the  point  comes  close  to  some  surface.    These 
precautions  result  in  the  distance  from  the  point  to  a  surface  having  to  be  totally 
recomputed  every  few  hundred  timesteps,  in  exchange  for  not  having  to  continually 
track the point on each surface. 
To track the point on the nearest surface, a 2D form of Newton's method is used.  The 
vector  function  to  be  solved  specifies  that  the  displacement  vector from  the  surface  to 
the point should be parallel to the surface normal vector.  The surface tangent vectors 
are  computed  with  respect  to  each  of  the  two  surface  patch  parameters,  and  the  dot 
product taken with the displacement vector.  See Figure 29.31 and Equation (29.104).   
(𝐩 − 𝐪) ⋅
∂𝐪
∂s
= 0 and (𝐩 − 𝐪) ⋅
∂𝐪
∂t
= 0.
(29.105)
This vector equation is then solved using Newton's method as in Equation (1.106).   
𝐪𝑖+1 = 𝐪𝑖 − (𝐅′)−1𝐅,
(29.106)
where
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
previous location
new location
new nearest point
previous nearest
point
Figure  29.32.   Newton iteration solves for the nearest  point on  the analytical
surface. 
𝐅(𝑠, 𝑡) =
⎜⎜⎜⎜⎜⎛(𝐩 − 𝐪) ⋅
(𝐩 − 𝐪) ⋅
⎝
⎟⎟⎟⎟⎟⎞
∂𝐪
∂𝑠
∂𝐪
∂𝑡 ⎠
. 
(29.107)
The convergence is  damped in the sense that the surface point is  not allowed to jump 
completely outside of a surface patch in one iteration.  If the iteration point tries to leave 
a  patch,  it  is  placed  in  the  neighboring  patch,  but  on  the  adjoining  boundary.    This 
prevents the point from moving merely continuous (i.e., when the surface has a crease 
in it).  Iteration continues until the maximum number of allowed iterations is reached, 
or  a  convergence  tolerance  is  met.    The  convergence  tolerance  (as  measured  in  the 
surface patch parameters) varies from patch to patch, and is based on the size and shape 
of  the  patch.    The  convergence  criterion  is  set  for  a  patch  to  ensure  that  the  actual 
surface point has converged (in the spatial parameters x, y, and z) to some tolerance. 
29.18  Simulated Draw Beads 
The  implementation  of  draw  beads  is  based  on  elastic-plastic  interface  springs  and 
nodes-to-surface  contact.    The  area  of  the  blank  under  the  draw  bead  is  taken  as  the 
master surface.  The draw bead is defined by a consecutive list of nodes that lie along the 
draw bead.  For straight draw beads only two nodes need to be defined, but for curved 
beads  sufficient  nodes  must  be  used  to  define  the  curvature.    The  draw  bead  line  is
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
integration points along drawbead line
points 1, 2, 3, and 4 define drawbeads
Figure  29.33.    The  drawbead  contact  provides  a  simple  way  of  including
drawbead behavior without the necessity of defining a finite element mesh for 
the drawbeads.  Since the draw bead is straight, each bead is defined by only
two nodes. 
discretized into points that become the slave nodes to the master surface.  The spacing 
of the points is determined by LS-DYNA such that several points lie within each master 
segment.  This is illustrated in Figure 29.32.  The dense distribution of point leads to a 
smooth  draw  bead  force  distribution  which  helps  avoid  exciting  the  zero  energy 
(hourglass)  modes  within  the  shell  elements  in  the  workpiece.    A  three-dimensional 
bucket search is used for the contact searching to locate each point within a segment of 
the master surface. 
The  nodes  defining  the  draw  beads  can  be  attached  to  rigid  bodies  by  using  the  extra 
nodes for rigid body input option.  When defining draw beads, care should be taken to 
limit the number of elements that are used in the master surface definition.  If the entire 
blank  is  specified  the  CPU  cost  increases  significantly  and  the  memory  requirements 
can become enormous.  An automated draw bead box, which is defined by specifying 
the part ID for the workpiece and the node set ID for the draw bead, is available.  The 
automated box option allows LS-DYNA determine the box dimensions.  The size of this 
box  is  based  on  the  extent  of  the  blank  and  the  largest  element  in  the  workpiece  as 
shown if Figure 29.34.   
The input for the draw beads requires a load curve giving the force due to the bending 
and  unbending  of  the blank  as  it  moves  through  the  draw  bead.    The  load  curve  may 
also include the effect of friction.  However, the coulomb friction coefficients must be set 
to zero if the frictional component is included in the load curve.  If the sign of the load 
curve ID is positive the load curve gives the retaining force per unit draw bead length 
as  a  function  of  displacement,  δ.    If  the  sign  is  negative  the  load  curve  defines  the
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
Figure  29.34.    The  draw  bead  box  option  automatically  size  the  box  around
the draw bead.  Any segments within the box are included as master segments
in the contact definition. 
maximum  retaining  force  versus  the  normalized  position  along  the  draw  bead.    This 
position varies from 0 (at the origin) to 1 (at the end) along the draw bead.  See Figures 
29.35 and 29.36. 
When friction is active the frictional force component normal to the bead in the plane of 
the work piece is computed.  Frictional forces tangent to the bead are not allowed.  The 
second  load  curve  gives  the  normal  force  per  unit  draw  bead  length  as  a  function  of 
displacement, δ.  This force is due to bending the blank into the draw bead as the binder 
closes on the die and  represents a limiting value.  The normal force begins to develop 
when the distance between the die and binder is less than the draw bead depth. As the 
binder  and  die  close  on  the  blank  this  force  should  diminish  or  reach  a  plateau.    This 
load curve was originally added to stabilize the calculation. 
As  the  elements  of  the  blank  move  under  the  draw  bead,  a  plastic  strain  distribution 
develops  through  the  shell  thickness  due  to  membrane  stretching  and  bending.    To 
account for this strain profile an optional load curve can be defined that gives the plastic 
strain  versus  the  parametric  coordinate  through  the  shell  thickness  where  the 
parametric  coordinate  is  defined  in  the  interval  from  –1  to  1.    The  value  of  the  plastic 
strain at each through thickness integration point is interpolated from this curve.  If the 
plastic  strain  at  an  integration  point  exceeds  the  value  of  the  load  curve  at  the  time 
initialization  occurs,  the  plastic  strain  at  the  point  will  remain  unchanged.    A  scale 
factor  that  multiplies  the  shell  thickness  as  the  shell  element  moves  under  the  draw 
bead can also be defined as a way of accounting for any thinning that may occur.
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
positive load curve ID
Penetration distande, δ
negative load curve ID
Normalized draw bead length
Figure 29.35.  Draw bead contact model defines a resisting force as a function
of draw bead displacement. 
29.19  Edge to Edge Contact 
Edge to edge contact can be important in some simulations.  For example, if a fan blade 
breaks away from the hub in a jet turbine contact with the trailing blade will likely be 
along the edges of the blades.  Edge to edge contact requires a special treatment since 
the nodal points do not make contact with the master segment which is the basis of the 
conventional contact treatments.  Currently all automatic type contact possess edge-to-
edge capabilities and therefore contact type 22 is only useful with those contact that do 
not possess this capability.  All contact using the segment-based formulation have edge 
to edge capabilities.
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
D, depth of draw bead 
F = Ffriction +Fbending
Figure 29.36.  Draw bead contact model defines a resisting force as a function 
of draw bead displacement. 
The basis of single edge contact is the proven single surface formulation and the input is 
identical.  The definition is by material ID.  Edge determination is automatic.  It is also 
possible to use a manual definition by listing line segments.  The single edge contact is 
type 22 in the structured input or *CONTACT_SINGLE_EDGE in the keyword input.
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
Figure  29.37.    Contact  between  edges  requires  a  special  treatment  since  the 
nodes do not make contact. 
This contact only considers edge to edge contact of the type illustrated in Figure 29.38.  
Here the tangent vectors to the plane of the shell and normal to the edge must point to 
each other for contact to be considered. 
29.20  Beam to Beam Contact 
In  the  beam  to  beam  contact  the  contact  surface  is  assumed  to  be  the  surface  of  a 
cylinder as shown in Figure 29.39.  The diameter of the contact cylinder is set equal to 
tangent vectors in 
plane of shell
Figure 29.38.  Single edge contact considers contact between two edges whose 
normals point towards each other. 
the  square  root  of  the  area  of  the  smallest  rectangle  that  contains  the  cross  section  to
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
avoid  tracking  the  orientation  of  the  beam  within  the  contact  algorithm.    Contact  is 
found by finding the intersection point between nearby beam elements and checking to 
see  if  their  outer  surfaces  overlap  as  seen  in  Figure  29.40.    If  the  surfaces  overlap  the 
contact  force  is  computed  and  is  applied  to  the  nodal  points  of  the  interacting  beam 
elements. 
Actual beam cross section
Contact surface
Figure 29.39.  Beam contact surface approximation. 
intersection point where forces are applied
Figure 29.40.  The forces are applied at the intersection point.
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
29.21  Mortar Contact 
The  Mortar  contact  was  originally  implemented  as  a  forming  contact  intended  for 
stamping  analysis  but  has  since  then  evolved  to  become  a  general  purpose  contact 
algorithm  for  implicit  time  integration.    The  Mortar  option  is  today  available  for 
automatic  single-  and  surface-to-surface  contacts  with  proper  edge  treatment,  beam 
contact, and optional features include tie, tiebreak and interference.  Contact is often the 
one  feature  that  overturns  the  implicit  performance,  so  to  facilitate  debugging  of  the 
Mortar  contacts  there  is  substantial  information  on  penetrations  written  to  the  LS-
DYNA  message  files.    The  Mortar  contact  is  a  penalty  based  segment-to-segment 
contact with finite element consistent coupling between the non-matching discretization 
of  the  two  sliding  surfaces  and  the  implementation  is  based  on  Puso  and  Laursen 
[2004a,b].    This  consistency,  together  with  a  differentiable  penalty  function  for 
penetrating  and  sliding  segments,  assert  the  continuity  and  (relative)  smoothness  in 
contact  forces  that  is  appealing  when  running  implicit  analyses.    The  algorithm  is 
primarily focusing on accuracy and robustness, and the involved calculations associated 
with  this  aim  make  it  expensive  enough  to  be  first  and  foremost  recommended  for 
implicit analysis.  There are numerous details in the implementation that simply cannot 
be explained without making the presentation incomprehensible, the intention here is to 
summarize  the  general  concepts  of  the  theory  behind  the  implementation  and  draw 
upon this to make some general recommendations on usage. 
29.21.1  Kinematics 
The  Mortar  contact  is  theoretically  treated  as  a  generalized  finite  element  where  each 
element in this context consists of a pair of contact segments.  The friction model in the 
ns
Ts
Slave segment
X3 X2
X1
Master Segment
Figure 29.41.  Illustration of Mortar segment to segment contact 
Mortar  contact  is  a  standard  Coulomb  friction  law.    Each  of  the  two  segments  has  its
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
iso-parametric representation inherited from the underlying finite element formulation, 
so the coordinates for the slave and master segments can be written  
𝒙𝑠 = 𝑁𝑠
𝒙𝑚 = 𝑁𝑚
𝑖(𝜉 , 𝜂) {𝒙𝑖 +
𝑗 (𝜉 , 𝜂) {𝒙𝑗 +
𝑡𝑠𝒏𝑠}
𝑡𝑚𝒏𝑚},
(29.21.108)
where  summation  over  repeated  indices  is  implicitly  understood,  i.e.,  over  the  nodes.  
We here also account that the contact surface may be offset from the mid-surface of e.g. 
shells,  in  the  direction  of  the  normal,  𝒏𝑠  and  𝒏𝑚,  by  half  the  thickness,  𝑡𝑠  and  𝑡𝑚.  The 
kinematics for the contact element can be written as the penetration 
𝑑 = 𝒏𝑠
𝑇(𝒙𝑠 − 𝒙̅𝑚),
(29.21.109)
where  𝒏𝑠  is  the  slave  segment  normal  and  𝒙̅𝑚  is  the  projected  point  on  the  master 
segment  along  the  slave  segment  normal.    The  element  is  only  defined  for  the 
intersection  between  the  slave  and  master  segment  and  for  points  where  𝑑 > 0,  this 
domain is denoted 𝛱 and is illustrated by gray in the Figure above.  The sliding rate 𝒔̇ is 
similarly defined as 
𝒔̇ = 𝑻𝑠
𝑇(𝒙̇𝑠 − 𝒙̅
̇𝑚),
where 𝑻𝑠 are two co-rotational basis vectors pertaining to the slave segment. 
29.21.2  Constitutive relation 
The contact pressure is given by the constitutive law 
𝜎n = 𝛼𝛽𝑠𝛽𝑚𝜀𝐾s𝑓 (
𝜀𝑑𝑐
𝑠),
(29.21.110)
(29.21.111)
where 
𝛼 = stiffness scaling factor (SFS*SLSFAC) 
𝐾s = stiffness modulus of slave segment 
𝜀 = 0.03 
𝑠 = characteristic length of slave segment 
𝑑𝑐
𝛽𝑠 = stiffness scale factor of slave segment (=1 unless specifically stated) 
𝛽𝑚 = stiffness scale factor of master segment (=1 unless specifically stated) 
and 
𝑓 (𝑥) =
⎧
{
{
⎨
{
{
⎩
𝑥2
cubic function that depends on IGAP
𝑥 <
𝑑max
2𝜀𝑑𝑐
𝑑max
2𝜀𝑑𝑐
𝑠 ≤ 𝑥
. 
(29.21.112)
where 𝑑max is the maximum penetration to be given below.  The Coulomb friction law 
is expressed in terms of the tangential contact stress
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
where 𝜇 is the friction coefficient and 
𝝈𝑡 = 𝜇𝜎𝑛
|𝒔|
𝑔 (
|𝒔|
𝜇𝑑
), 
(29.21.113)
𝑔(𝑥) =
⎧
{{
⎨
{{
⎩
𝑥 ≤ 1 − 𝜀
1 −
(
1 + 𝜀 − 𝑥
)
1 − 𝜀 < 𝑥 ≤ 1 + 𝜀
. 
(29.21.114)
1 + 𝜀 < 𝑥
The update of 𝒔 is done incrementally and is at the end of the step modified so that 
|𝒔| ≤ 𝜇𝑑(1 + 𝜀)
(29.21.115)
after the contact update. 
29.21.3  Contact nodal forces 
From  the  contact  stress,  the  contact  nodal  forces  are  determined  by  the  principle  of 
virtual work 
𝑖 = 𝛿𝑖
𝒇𝑠
𝑘 {𝑰 +
𝑡𝑠
} {𝒏𝑠 ∫ 𝑁𝑠
𝑘𝜎𝑛𝑑𝛱
+ 𝑻𝑠 ∫ 𝑁𝑠
𝑘𝝈𝑡𝑑𝛱
}
(29.21.116)
𝑗 = 𝛿𝑗
𝒇𝑚
𝑘 {𝑰 +
𝑡𝑚
} {−𝒏𝑠 ∫ 𝑁𝑚
𝑘 𝜎𝑛𝑑𝛱
− 𝑻𝑠 ∫ 𝑁𝑚
𝑘 𝝈𝑡𝑑𝛱
}, 
𝜕𝒏𝑠
𝜕𝒙𝑘
𝜕𝒏𝑚
𝜕𝒙𝑘
where the subscript 𝑠 and 𝑚 stands for the slave and master nodal forces, respectively, 
and 𝛿 denotes the Kronecker delta.  Worth noting here is that accounting for offsets in 
the  kinematic  description  leads  to  a  term  that  will  induce  a  torque  due  to  frictional 
tractions.  To this end, we need to remark that the kinematics for shell edges do not fall 
into  the  framework  presented  here;  the  actual  map  between  the  nodal  and  segment 
coordinates  is  not  accounted  for  and  contact  traction  will  in  those  cases  only  induce 
translational  forces  on  the  nodes  along  the  edge.    For  beams,  nodal  rotations  are 
involved  in  the  kinematics  and  frictional  torques  are  accounted  for  but  in  a  different 
way. 
29.21.4  Treatment of beams, sharp solid and shell edges 
The automatic Mortar contacts support contact with the lateral surface and end tips of 
beams  as  well  as  edges  of  shell  elements  and  sharp  edges  of  solids.    The  concept  of 
sharp  solid  edges  will  be  defined  below.    The  theory  presented  above  is  in  this  case 
applied  to  dummy  segments  corresponding  to  a  faceted  representation  of  the  beam 
lateral surface and the edges of the solid and shell elements, respectively, as indicated in 
Figure  29-42.  For  a  beam  element  the  contact  surface  is  represented  by  14  faceted 
segments  encapsulating  a  cylinder  with  the  same  length  and  volume  as  the  beam 
element itself.  This implies that all beam elements are assumed to have a circular cross 
section for the contact.  The edges of the shell element surface are identified assuming 
the  user  contact  definition  (slave  or  master)  consists  of  the  entire  physical  component 
(metal sheet) in question.  It is therefore recommended to  
•Define the contacts using part or part sets or otherwise false edges may be created 
in the interior of the component.
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
An  edge  contact  element  is  created  by  extruding  the  shell  edge  in  the  direction  of  the 
shell  normal  by  a  distance  corresponding  to  the  shell  thickness  with  appopriate 
adjustments  for  irregular  geometries.    As  mentioned  above, the  kinematics  in  creating 
these  edge  segments  do  not  account  for  its  numerical  representation  and  whence  the 
Mortar contact does not assemble the corresponding forces in a finite element consistent 
manner.    The  shell  edge  treatment  is  to  be  seen  as  a  simplified  treatment  just  to 
incorporate  a  contact  resistance  for  these  geometries,  which  is  probably  ok  in  most 
practical  situations.    For  beam  elements  however,  rotational  degrees  of  freedom  are 
included in a consistent way, thus causing beam elements to rotate with respect to their 
axes when tangential friction forces are applied to the lateral surface.  A sharp solid edge 
is detected when the angle 𝜃 between the normals of two adjacent contact segments is 
larger than 𝜋/3, and in this case the edge is smoothed by adding 4 segments between 
the two nodes common to the two contact segments, while at the same time adjusting 
the size of the two main contact segments.  The effect is a rounded representation of the 
edge and a smoother contact response, see Figure 29-42. The size of the smoothing is at 
most 5% of the size of the smallest of the two contact segments, so the effect is reduced 
with mesh refinement.  Since the contact area of these edge segments may be small, the 
stiffness of the  contact is for those scaled by the factor 𝛽 = √3cot (𝜋−𝜃
2 )  where 𝜃 is  the 
initial  angle  between  the  main  segment  normals.    This  scale  factor  is  applied  for  both 
the slave and master side, meaning that if two right angled edges come into contact the 
𝜋−𝜋
𝜋−𝜋
2 ) √3 cot (
stiffness is scaled by 𝛽𝑠𝛽𝑚 = √3 cot (
2 ) = 9. Whether this is sufficient to 
handle most common situations is currently unknown, so this design decision is subject 
for  change  in  the  future.    If  a  contact  segment  has  two  sharp  edges  with  a  common 
node, then a segment is created at the location of that node to account for contact with 
the corner of the solid element geometry.  The stiffness scale factor for a corner node is 
the average of the scale factor for the connected edges.  The motivation behind the solid 
edge  smoothing  is  two-fold;  for  one  thing  it  adds  the  feature  of  resisting  penetration 
between  a  solid  edge/corner  and other geometries  and  then  it  also aids  establishing  a 
physical  contact  state  when  solid  elements  slide  off  sharp  geometrical  objects.    More 
specifically  it  eliminates  the  ambiguity  of  which  contact  segments  are  in  contact  with 
which,  and  presumably  prevents  sudden  spikes  in  the  contact  force,  this  is  also 
illustrated in Figure 29-42. 
It is important to stress that the automatic Mortar contact surfaces are always located on 
the  outer  geometry  for  both  slave  and  master  sides,  i.e.,  contact  does  not  occur  on  the 
mid-surface of shells.  A common modelling problem is illustrated in Figure 29-43 that 
results  in  extremely  large  contact  stress  unless  the  ignore  flag  is  appropriately  used.  
The forming contact is treated differently not only in that shell edge or beam contact is 
not  supported.    Here  any  shell  master  surface  must  be  rigid  with  its  segment  normals 
oriented towards the slave side of the contact.  Furthermore the contact occurs here on 
the mid-surface in contrast to the automatic option, while contact on the slave side still 
occurs on the outer geometry.  The segment orientation of the (deformable) slave side is 
on one hand arbitrary, but if it consists of shell elements contact can only occur on one 
side  for  a  given  contact  definition.    In  a  forming  application  for  instance,  the  contact
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
between  the  tool  and  blank  and  the  contact  between  the  die  and  blank  have  to  be 
defined  using  two  different  contact  interfaces  since  these  contacts  typically  occur  on 
different sides of the blank.  Forming solid master surfaces may be rigid or deformable, 
thus allowing for effects of tool deformation and/or cooling effects.
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
Figure 29-42  29  Faceted  representation  of  beams  (including  4  quads
representing  a  tip  end),  shell  and  sharp  solid  edges,  respectively,  the
segment geometry indicated by red.  The contact surface representation
of three cubic solid elements is illustrated, with a somewhat exaggerated 
smoothing  for  illustration  purposes.    The  effect  of  edge  smoothing  in
contact is illustrated in a section cut bottom right, if the red objects slides
to  the  right  and  the  blue  objects  are  fixed,  the  sudden  detection  of  a 
parasitic  contact  indicated by  the double arrow results in  a  jump in the
contact force, this is alleviated by smoothing of the edges below.
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
Correct  modelling  if  IGNORE  is  used, 
master edge shows excessive penetration but 
contact surface is adjusted 
Incorrect modelling if IGNORE is not used, 
master  edge  shows  excessive  penetration, 
large contact stress 
Correct  modelling  regardless  of  IGNORE, 
master  edge  is  located  on  outer  surface  of 
slave segment, zero contact stress 
Figure  29-43  Intersected  view  of  shells  in  edge-to-surface  contact.    Shell  mid-
surfaces indicated by dashed lines, outer surfaces by solid lines.  Slave shell nodes 
are blue, master shell nodes are red and initial volume of penetration is shaded.
29.21.5  Characteristic length and contact release 
𝑠  and  𝑑𝑐
𝑚  of  the  slave  and  master  sides,  respectively,  are 
The  characteristic  lengths  𝑑𝑐
important  in  Mortar  contact  since  they  affect  the  contact  stiffness  but  also  because  it 
determines the maximum allowed penetration between two arbitrary segments.  To be 
more  specific,  two  segments  cannot  penetrate  more  than  95%  of  the  average 
characteristic  lengths,  penetrations  larger  than  that  will  not  be  detected. 
  In 
mathematical terms this can be stated as 
𝑑max = 0.95
𝑠 + 𝑑𝑐
𝑑𝑐
(29.117)
𝑠  is  the  characteristic  length  of  the  slave 
where  𝑑max  is  the  maximum  penetration,  𝑑𝑐
𝑚 is the characteristic length of the master segment.  This is illustrated in 
segment and 𝑑𝑐
Figure  29.44  that  shows  the  contact  stress  as  function  of  the  relative  penetration.    To 
minimize  the  risk  of  releasing  contacts  one  could  increase  the  stiffness  parameter  SFS, 
but  this  may  lead  to  worse  convergence  in  implicit  analysis.    To  this  end,  the  IGAP 
parameter  can  be  used  to  stiffen  the  contact  for  large  penetrations  without  affecting 
moderate  penetrations,  this  is  also  illustrated  in  Figure  29.44  and  can  be  used  if  the 
contact pressure is locally very high.  This also highlights the following important fact:  
The Mortar contact has no “stick” option for improving implicit convergence.
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
 4
 3.5
 3
 2.5
 2
 1.5
 1
 0.5
 0
 0
IGAP=1 
IGAP=2 
IGAP=5 
IGAP=10
 0.2
 0.4
 0.6
 0.8
 1
Penetration
  Figure 29.44. Mortar contact stress as function of penetration relative 2𝑑max. 
This may on one hand lead to worse convergence characteristics but on the other rules 
out sticky behavior and underreport of contact forces in the ascii database.  
The characteristic length is for shells the shell thickness, whereas for solids it is a 
smaller  element  size  in  the  part  that  the  segment  belongs  to.    The  latter  may  lead  to 
unrealistically  high  or  low  contact  stiffness,  or  it  may  result  in  a  too  small  maximum 
penetration  depth,  all  depending  on  the  mesh.    For  this  reason  the  user  may  set 
PENMAX  to  the  characteristic  length,  which  should  correspond  to  some  physical 
member size in the model, and/or adjust the contact stiffness, depending on what the 
issue is. 
29.21.6  Outputs for debugging implicit models 
In implicit analysis it is almost inevitable to run into convergence problems, especially 
when contacts are involved.  When this happens the user usually craves for information 
on  what’s  gone  wrong.    For  the  Mortar  contact,  detailed  information  on  penetration 
distance and potential contact release (i.e., penetration becomes too large for the contact 
to  be  detected  in  subsequent  steps)  can  be  requested  through  MINFO = 1  on  CON-
TROL_OUTPUT. With this option information on largest penetration, both absolute and 
relative, is given in the message files after each converged step, including a warning if 
penetration  is  close  to  being  released.    It  also  reports  the  elements  with  largest 
penetrations  which  makes  it  easy  to  locate  critical  areas  of  the  model  in  LS-PrePost.  
Contact release should be avoided or otherwise results may be useless. 
On the other side of the spectrum, poor convergence could be due to a too stiff 
contact.  Since the stiffness for a Mortar contact segment pair only depends on the slave 
segment it is recommended to
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
Contact surface augment SLDTHK 
Contact surface augment (SST × SFST-T)/2 
Element thickness T 
Figure  29.45.    Illustration  of  contact  surface  location  for  automatic  Mortar
contact, solids on top and shells below. 
•Put weak parts on the slave side 
If  a  steel  part  is  in  contact  with  rubber  for  instance,  the  rubber  part  should  be  put  as 
slave  side  in  the  contact  definition.    One  way  of  find  contacts  that  cause  poor 
convergence  in  implicit  is  to  turn  on  D3ITCTL  on  CONTROL_IMPLICIT_SOLUTION 
and RESPLT on DATABASE_EXTENT_BINARY, which allows the user to isolate areas 
in the model where convergence is poor.  Not rarely this is due to contacts.  
29.21.7  Initial penetrations 
Initial  penetrations  are  always  reported  in  the  message  files,  including  the  maximum 
penetration and how initial penetrations are to be handled.  The IGNORE flag governs 
the latter and the options are 
IGNORE < 0 
IGNORE = 0 
IGNORE = 1 
IGNORE = 2 
IGNORE = 3 
See  explanation  for  the  corresponding  positive  value,  the  only 
difference  is  that  contact  between  segments  belonging  to  the  same 
part is not treated 
Initial  penetrations  will  give  rise  to  initial  contact  stresses,  i.e.,  the 
slave  contact  surface  is  not  modified,  this  option  is  not  available  for 
Mortar contact but defaults to IGNORE = 2 
Initial  penetrations  will  be  tracked,  i.e.,  the  slave  contact  surface  is 
translated  to  the  level  of  the  initial  penetrations  and  subsequently 
follow the master contact surface on separation until the unmodified 
level is reached  
Initial  penetrations  will  be  ignored,  i.e.,  the  slave  contact  surface  is 
translated  to  the  level of  the  initial  penetrations,  optionally  with  an 
initial contact stress governed by MPAR1, this is the default option for 
Mortar contact 
Initial penetrations will be removed over time, i.e., the slave contact 
surface  is  translated  to  the  level  of  the  initial  penetrations  and 
pushed  back  to  its  unmodified  level  over  a  time  determined    by 
MPAR1
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
IGNORE = 4 
Same  as  IGNORE = 3  but  it  allows  for  large  penetrations  by  also 
setting MPAR2 to at least the maximum initial penetration 
The  use  of  IGNORE  depends  on  the  problem,  if  no  initial  penetrations  are 
present there is no need to use this parameter at all.  If penetrations are relatively small 
in  relation  to  the  maximum  allowed  penetration,  then  IGNORE = 1  or  IGNORE = 2 
seems  to  be  the  appropriate  choice.    For  IGNORE = 2  the  user  may  specify  an  initial 
contact  stress  small  enough  to  not  significantly  affect  the  physics  but  large  enough  to 
eliminate rigid body modes and thus singularities in the stiffness matrix.  The intention 
with this is to constrain loose parts that are initially close but not in contact by pushing 
out  the  contact  surface  using  SLDTHK  or  SFST  and  applying  the  IGNORE = 2  option.  
Increasing  SFST  for  shells  to  a  number  larger  than  unity  will  push  the  contact  surface 
outside the geometry and contact will be detected accordingly, see Figure, the SLDTHK 
parameter  is  used  for  solids.    It  is  at  least  good  for  debugging  problems  with  many 
singular rigid body modes. 
IGNORE = 3 is the Mortar interference counterpart, used for instance if there is a 
desire to fit a rubber component in a structure or for eliminating initial penetrations by 
simulation.  With this option the contact surfaces are restored linearly in time from the 
beginning  of  the  simulation  to  the  time  specified  by  MPAR1.  If  the  intention  is  to 
initial  penetrations  completely,  and  since  contact  penetrations  are 
eliminate 
unavoidable  to  some  extent,  it  may  also  in  this  case  be  of  importance  to  use  SFST  or 
SLDTHK  to  reduce  the  possibility  that  the  actual  geometry  is  penetrated.    If  using  a 
single surface definition on a complicated geometry with many parts, a negative value 
of IGNORE could be of interest, since the Mortar contact may otherwise detect spurious 
contacts between segments belonging to the same part. 
A  drawback  with  IGNORE = 3  is  that  initial  penetration  must  be  smaller  than 
half the characteristic length of the contact or otherwise they will not be detected in the 
first place.  For this reason IGNORE = 4 was introduced where initial penetrations may 
be of arbitrary size, but it requires that the user provides crude information on the level 
of  penetration  of  the  contact  interface.    This  is  done  in  MPAR2  which  must  be  larger 
than  the  maximum  penetration  or  otherwise  an  error  termination  will  occur.  
IGNORE = 4 only applies to solid elements at the moment.
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
𝑠1 
𝑠2
𝑚2
𝑚1 
𝑠1 vs 𝑚2  
𝒙1 
𝑠1 vs 𝑚1  
𝑑(𝑡)
𝒏𝑠
𝒚1
𝒙(𝑡)
𝒙2
𝒚(𝑡)
𝒏𝑚
𝒕 
𝒚2 
𝑠2 vs 𝑚2  
29-4629  2D  mortar  contact,  2  slave  segments  in  contact  with  2  master 
segments results in three separate treatments. 
29.21.8  2D Mortar contact 
Automatic single and surface-to-surface Mortar contact is available and here described 
in detail as an attempt to illustrate it in a setting that is hopefully easier to understand.  
In Figure 29-46 (top) the contact between 2 slave and 2 master segments is shown as an 
example.    This  particular  configuration  results  in  the  treatment  of  3  slave  vs  master 
contact pairs (bottom), and for the mathematical treatment we refer to this figure as an 
illustration. 
Kinematics 
First a common tangential direction is determined, this is given as 
𝒕 =
𝒙2 + 𝒚2 − 𝒙1 − 𝒚1
∥𝒙2 + 𝒚2 − 𝒙1 − 𝒚1∥
(29.118)
and the corresponding normal 𝒏 is perpendicular to 𝒕, with the direction convention as 
illustrated.  We can define a coordinate 𝑡 along this tangential direction, the origin can 
be chosen arbitrarily, and then 𝒙(𝑡) and 𝒚(𝑡) are the projection coordinate along 𝒏 onto 
the  slave  and  master  segment,  respectively.    Obviously  there  is  a  finite  interval    𝑡 ∈
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
[𝑡 ̃1, 𝑡 ̃2] where both 𝒙(𝑡) and 𝒚(𝑡) is well-defined, and on this interval we can define the 
penetration as 
𝑑(𝑡) = 𝒏𝑇(𝒙(𝑡) − 𝒚(𝑡)). 
(29.119)
The  overlapped  interval  is  then  further  reduced  to  𝑡 ∈ [𝑡1, 𝑡2]  for  which  𝑑(𝑡) ≥ 0,  note 
that for the 𝑠2 vs 𝑚2 situation these two intervals are not the same.  The interval [𝑡1, 𝑡2] is 
indicated  by  red  in  the  illustration.    This  completes  the  kinematics  in  the  normal 
direction. 
In the tangential direction we need to define the kinematics for sliding and we do this 
by  associating  a  history  variable  to  each  slave  segment.    To  this  end,  𝑆  as  a  weighted 
measure of the distance a slave segment has slid along the master surface and is defined 
as 
𝑆 = 𝑆𝑛−1 + ∑ ∫ {𝑠(𝑡) − 𝒕𝑛−1
𝐴𝑖
𝑇 (𝒙𝑛−1(𝑡) − 𝒚𝑛−1(𝑡))}𝑑𝐴𝑖
(29.120)
where 𝑠(𝑡) = 𝒕𝑇(𝒙(𝑡) − 𝒚(𝑡)) and the subscript 𝑛 − 1 refers to the corresponding value in 
the previous step.  The integral is taken over the domain 𝐴𝑖 of the intersected interval 
between  the  slave  segment  and  master  segment  𝑖,  accounting  for  plane  strain  or  axial 
symmetry.  Note that the slave segment can be in contact with several master segments, 
whence  the  sum.    Further  noting  that  by  construction  the  first  term  in  the  integrand, 
𝑠(𝑡) = 0, we can simplify this to 
𝑆 = 𝑆𝑛−1 − ∑ ∫ 𝒕𝑛−1
𝑇 (𝒙𝑛−1(𝑡) − 𝒚𝑛−1(𝑡))𝑑𝐴𝑖
𝐴𝑖
. 
(29.121)
In the illustrated situation, slave segment 1 would get sliding contributions from master 
segments  1  and  2,  while  slave  segment  2  only  from  master  segment  2.  Likewise  we 
define a weighted penetration 
which is used together with 𝑆 to define the friction law below. 
𝐷 = ∑ ∫ 𝑑(𝑡)𝑑𝐴𝑖
𝐴𝑖
. 
(29.122)
Constitutive relations 
For  simplicity,  we  drop  the  explicit  dependence  on  𝑡  from  now  on  and  define  the 
contact stress (pressure) as 
where 𝐾 is the contact stiffness defined as 
𝜎𝑛 = 𝐾 𝑑2
𝐾 =
0.01
𝑇𝑠𝑇𝑚
2𝐾𝑠𝐾𝑚
𝐾𝑠 + 𝐾𝑚
𝑓 (𝒏𝑠
𝑇𝒏𝑚). 
(29.123)
(29.124)
Furthermore,  𝛼 = PSF ∗ SLSFAC  is  a  stiffness  scale  factor  and  𝑇𝑠/𝑚  and  𝐾𝑠/𝑚  are 
characteristic  lengths  and  material  stiffnesses  of  the  slave  and  master  segments, 
respectively.  The function 𝑓  is used to linearly reduce stiffness for segments that are not 
parallel, note that 𝒏𝑠 and  𝒏𝑚 are the normals to the slave and  master segments, and is 
given as
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
⎧
{
{
{
{
{
⎨
{
{
{
{
{
⎩
The friction stress is defined as 
𝑓 (𝑥) =
−
≤ 𝑥
1 + 2𝑥
1 − √3
−
√3
≤ 𝑥 < −
. 
𝑥 < −
√3
(29.125)
𝜇𝐷
with  𝜇  being  the  Coulomb  friction  coefficient  and  𝑔  is  a  continuously  differentiable 
function defined as 
𝜎𝑡 = 𝜇𝜎𝑛𝑔 (
(29.126)
) 
𝑔(𝑥) =
⎧
{{{{{
{{{{{
⎨
⎩
1 −
25
1,
𝑥 ≥ 1.03
(𝑥 − 1.03)2,
0.97 ≥ 𝑥 > 1.03
𝑥, −0.97 ≥ 𝑥 > 0.97
−1 +
25
(𝑥 + 1.03)2, −1.03 ≥ 𝑥 > −0.97
−1,
−1.03 > 𝑥
(29.127)
The interpretation of this law is that the magnitude of friction stress 𝜎𝑡 is at most 𝜇𝜎𝑛, 
and  the  fraction  thereof  is  determined  by  the  appropriate  relation  between  the 
accumulated  sliding  and  penetration.    Upon  convergence,  to  yield  a  proper  friction 
behavior, 
𝑆𝑛 =
the 
updated 
max (−1.03𝜇𝐷, min(1.03𝜇𝐷, 𝑆)). 
according 
next 
step 
for 
to 
is 
𝑆 
Nodal forces 
The  nodal  force  contribution  from  a  given  segment  pair  is  determined  from  the 
principle of virtual work, i.e.,  
𝛿𝑊 = ∫ 𝜎𝑛 𝛿𝑑 𝑑𝐴
. 
+ ∫ 𝜎𝑡 𝛿𝑠 𝑑𝐴
(29.128)
Here 𝛿 is the variation operator, and the independent variables subject to this variation 
are  the  nodal  coordinates.    Thus,  replacing  the  left  hand  side  with  the  expression 
involving  nodal  forces  and  coordinates,  and  using  (29.123)  and  (29.126)  for  the  right 
hand side we get 
∑ 𝒇𝐼
𝑇𝛿𝒙𝐼
= 𝐾 ∫ 𝑑2 𝛿𝑑 𝑑𝐴
+ 𝜇𝐾𝑔 ∫ 𝑑2 𝛿𝑠 𝑑𝐴
. 
The nodal forces are then readily identified as 
𝒇𝐼 = 𝐾 ∫ 𝑑2  
𝜕𝑑
𝜕𝒙𝐼
𝑑𝐴
+ 𝜇𝐾𝑔 ∫ 𝑑2 𝜕𝑠
𝜕𝒙𝐼
. 
𝑑𝐴
(29.129)
(29.130)
where  the  exact  expressions  for  the  integrals  in  terms  the  nodal  coordinates  are, 
although straightforward to derive, a bit lengthy and therefore omitted. 
Stiffness matrix
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
The  stiffness  matrix  is  the  second  variation  of  the  virtual  work  expression  (29.128) 
where we neglect the variation of the overlapped area and assume the variation can be 
taken on the integrand directly 
∆𝛿𝑊𝐼 = 2𝐾 ∫ 𝑑 ∆𝑑 𝛿𝑑 𝑑𝐴
𝜇𝐷
𝜕𝑔
𝜕𝑥
+ 𝜇
{
+ 2𝜇𝐾𝑔 ∫ 𝑑 ∆𝑑 𝛿𝑠 𝑑𝐴
∆𝑆 −
. 
𝜇𝐷2 ∆𝐷} ∫ 𝜎𝑛 𝛿𝑠 𝑑𝐴
(29.131)
Here  ∆  is  again  the  variation  operator,  different  notation  to  distinguish  it  from  𝛿  but 
performing the exact same thing.  At this point we emphasize that the (geometric) terms 
involving ∆𝛿𝑑 and ∆𝛿𝑠 have been deliberately excluded as they, albeit being symmetric, 
contribute to the indefiniteness of the tangent matrix.  In (29.131), the first term on the 
right hand side is the normal-normal interaction and is nicely symmetric, the remaining 
terms  come  from  friction  (normal-tangent  and  tangent-tangent  interaction)  and  needs 
symmetrization and further simplification.  To this end we neglect any terms involving 
∆𝑑 𝛿𝑠 and ∆𝐷𝛿𝑠 which means that it remains to deal with the term involving ∆𝑆 𝛿𝑠. The 
simplifications made are to approximate 
∫ 𝜎𝑛 𝑑𝐴
in  the  last  integral,  and  then  neglect  all  terms  in  ∆𝑆  that  do  not  pertain  to  the  present 
slave master segment pair.  This results in  
𝜎𝑛 ≈
(29.132)
∆𝒙𝐼
𝑇𝑲𝐼𝐽
𝑇𝛿𝒙𝐽 ≈ 2𝐾 ∫ 𝑑 ∆𝑑 𝛿𝑑 𝑑𝐴
and the stiffness matrix can be identified as 
𝜕𝑔
𝜕𝑥
+
{
∫ 𝜎𝑛 𝑑𝐴
} {∫ ∆𝑠 𝑑𝐴
} {∫ 𝛿𝑠 𝑑𝐴
} 
(29.133)
𝑲𝐼𝐽 = 2𝐾 ∫ 𝑑 
𝜕𝑑
𝜕𝒙𝐼
𝜕𝑑
𝜕𝒙𝐽
 𝑑𝐴
+
𝜕𝑔
𝜕𝑥
{
∫ 𝜎𝑛 𝑑𝐴
} {∫
𝜕𝑠
𝜕𝒙𝐼
𝑑𝐴
} {∫
𝜕𝑠
𝜕𝒙𝐽
 𝑑𝐴
}. 
(29.134)
A  characteristic  feature  of  the  Mortar  contact,  which  can  be  deduced  from  this 
expression, is that not only the nodal forces are continuous but also the stiffness matrix.  
This follows from the 𝐶1 continuity of 𝑔, meaning that all involved functions above are 
continuous,  and  that 𝑲𝐼𝐽  tends  to  zero  as  either  𝑑  or 𝐴  tends  to  zero.   A  mathematical 
treatment yields 
∥𝑲𝐼𝐽∥ ≤ 𝐾𝐴 max
𝑑(𝑡) {2 max
𝜕𝑑(𝑡)
∥
𝜕𝒙𝐼
∥ ∥
𝜕𝑑(𝑡)
𝜕𝒙𝐽
∥ + max
∥
𝜕𝑠(𝑡)
𝜕𝒙𝐼
∥ ∥
𝜕𝑠(𝑡)
𝜕𝒙𝐽
∥} 
(29.135)
which  tends  to  zero  as  𝑑  or  𝐴  tends  to  zero  as  the  terms  inside  the  right  bracket  are 
bounded. 
29.21.9  Tied and tiebreak option 
A  tied  and  tiebreak  option  with  the  Mortar  contact  is  available  by  appending 
MORTAR_TIED  or  TIEBREAK_MORTAR  to  the  automatic  surface  to  surface  contact 
keyword.    In  principle,  the  tiebreak  allows  for  specifying  the  contact  stress  𝜎  as  a 
function of the separation 𝑑 to accomodate a given interface law that includes softening 
and failure (loss of interface stiffness).  The law incorporates both normal and tangential 
directions,  usually  denoted  mode  I  and  mode  II  in  the  delamination  community,  and 
the  typical  appearance  of  such  a  law  is  shown  in  Figure  bm_figcohlaw.  The  law  is  in
Contact-Impact Algorithm 
LS-DYNA Theory Manual 
general  characterized  by  the  energy  release  rate  𝐸  which  is  the  energy  per  unit  area 
required  to  release  the  contact,  and  the  maximum  interface  stress  𝜎𝑒  which  is  the  peak 
contact  stress  before  softening  begins.    Referring  to  the  above  mentioned  figure,  the 
energy  release  rate  is  the  integral  of  the  curve  describing  the  stress  vs  displacement 
relation.  The law can indeed be quite complicated, and we refer to the keyword manual 
for more information regarding details of the cohesive models available. For the Mortar 
tiebreak option only OPTION = 7 and OPTION = 9 are supported. The internal treatment of 
the Mortar tied and tiebreak options are very similar to that of the one-sided contacts, 
but the following remarks are in place. 
•Tied  Mortar  contact  is  penalty  based  and  exhibits  a  linear  relationship  between 
normal/tangential  separation  and  resulting  contact  stress.  In  referring  to  equa-
tion (29.21.111), 𝑓 (𝑥) = 𝑥 for all 𝑥 in all separation directions. Since the nonlineari-
ty  is  significantly  reduced  compared  to  one-sided  contacts,  the  implicit 
convergence characteristics are insensitive to scaling of the contact stiffness. 
•Tiebreak Mortar contact is treated similarly  but the normal and tangential contact 
stress is given by the constitutive model.  It is strongly recommended to set CN 
(OPTION = 7 and OPTION = 9) and CT2CN (only OPTION = 9) on the addition-
al  card  associated  with  the  tiebreak  option,  otherwise  the  interface  stiffness  is 
determined internally and may be inconveniently large. 
•Tiebreak Mortar contact is superposed by a one-sided contact to take compressive 
contact stress, mainly to prevent penetrations in the post-failure regime but also 
to prevent cohesive failure due to normal compression.  This contact follows the 
theory described above and automatically applies the IGNORE = 2 option to start 
with an initial zero contact stress. 
•The one-sided contact associated with the tiebreak option is frictionless as long as 
the  tied  contact  exists,  this  to  avoid  spurious  interactions  between  the  laws 
(mode  II  and  friction)  in  the  tangential  directions.    The  friction  is  activated  as 
soon as the tied contact is released.  Furthermore, the tied interface will not take 
compressive stress as this is lent to the one-sided contact.  
•Tied and tiebreak Mortar contacts are applied if the initial normal distance between 
the slave and master segment (with respect to their outer geometries) is less than 
a  critical  distance,  𝑑𝑡 = 0.05𝑑𝑐.  In  this  formula  𝑑𝑐  is  the  characteristic  length  as 
described above.  Here 𝑑𝑡 =PENMAX can be  used to override this tolerance for 
when  to  tie  two  segments,  so  the  meaning  of  PENMAX  is  in  this  case  different 
than for the unilateral contacts.
LS-DYNA Theory Manual 
Contact-Impact Algorithm 
Shear Contact Forces
Workpiece
Support
 150000
 100000
 50000
 0
-50000
-100000
-150000
 0
 10
 20
 30
 40
 50
 60
Workpiece Displacement
Figure  29-47  A  rubber  compression  example  solved  in  implicit  with  Mortar  contact 
(Courtesy  of  Dellner  Couplers  AB).    The  graph  shows  the  contact  force  between  the 
rubber  parts  and  the  moving  workpiece  and  between  the  rubber  parts  and  the  two 
supports, respectively.
LS-DYNA Theory Manual 
Geometric Contact Entities 
30    
Geometric Contact Entities 
Contact  algorithms  in  LS-DYNA  currently  can  treat  any  arbitrarily  shaped 
surface  by  representing  the  surface  with  a  faceted  mesh.    Occupant  modeling  can  be 
treated this way by using fine meshes to represent the head or knees.  The generality of 
the faceted mesh contact suffers drawbacks when modeling occupants, however, due to 
storage  requirements,  computing  costs,  and  mesh  generation  times.    The  geometric 
contact  entities  were  added  as  an  alternate  method  to  model  cases  of  curved  rigid 
bodies  impacting  deformable  surfaces.    Much  less  storage  is  required  and  the 
computational cost decreases dramatically when compared to the more general contact. 
Geometric  contact  entities  are  developed  using  a  standard  solids  modeling 
approach.    The  geometric  entity  is  defined  by  a  scalar  function  𝐺(𝑥, 𝑦, 𝑧).    The  solid  is 
determined from the scalar function as follows: 
𝐺(𝑥, 𝑦, 𝑧) > 0 The point (𝑥, 𝑦, 𝑧) is outside the solid
𝐺(𝑥, 𝑦, 𝑧) = 0 The point (𝑥, 𝑦, 𝑧) is on the surface of the solid 
𝐺(𝑥, 𝑦, 𝑧) < 0 The point (𝑥, 𝑦, 𝑧) is inside the solid
(30.1)
(30.2)
(30.3)
Thus,  by  a  simple  function  evaluation,  a  node  can  be  immediately  determined  to  be 
outside the solid or in contact.  Figure 30.1 illustrates this for a cylinder. 
If  the  node  is  in  contact  with  the  solid,  a  restoring  force  must  be  applied  to 
eliminate  further  penetration.    A  number  of  methods  are  available  to  do  this  such  as 
Lagrange multipliers or momentum based methods.  The penalty method was selected 
because  it  is  the  simplest  and  most  efficient  method.    Also,  in  our  applications  the 
impact velocities are at a level where the penalty methods provide almost the identical 
answer as the exact solution. 
Using the penalty method, the restoring force is proportional to the penetration 
distance into the solid and acts in the direction normal to the surface of the solid.  Thus,
Geometric Contact Entities 
LS-DYNA Theory Manual 
G(x, y) < 0
G(x, y) > 0
G(x, y) = 0
Figure  30.1.    Determination  of  whether  a  node  is  interior  or  exterior  to  the 
cylindrical surface 
the  penetration  distance  and  the  normal  vector  must  be  determined.    The  surface 
normal vector is conveniently determined from the gradient of the scalar function. 
𝐍(𝑥, 𝑦, 𝑧) =
∂𝐺
∂𝑥
𝐢 + ∂𝐺
∂𝑦
𝐣 + 𝜕𝐺
𝜕𝑧
, 
√(∂𝐺
)
∂𝑥
+ (∂𝐺
)
∂𝑦
+ (∂𝐺
∂𝑧
)
(30.4)
for  all  (𝑥, 𝑦, 𝑧)  such  that  𝐺(𝑥, 𝑦, 𝑧) = 0.    The  definition  of  𝐺(𝑥, 𝑦, 𝑧)  guarantees  that  this 
vector  faces  in  the  outward  direction.    When  penetration  does  occur,  the  function 
𝐺(𝑥, 𝑦, 𝑧)  will  be  slightly  less  than  zero.    For  curved  surfaces  this  will  result  in  some 
errors in calculating the normal vector, because it is not evaluated exactly at the surface.  
In  an  implicit  code,  this  would  be  important,  however,  the  explicit  time  integration 
scheme in DYNA3D uses such a small time step that penetrations are negligible and the 
normal function can be evaluated directly at the slave node ignoring any penetration. 
𝐺(𝑥, 𝑦) = 𝑥2 + 𝑦2 − 𝑅2,
(30.5)
The  penetrations  distance  is  the  last  item  to  be  calculated.    In  general,  the  penetration 
distance, 𝑑, is determined by. 
where  𝐗𝑛  is  the  location  of  node  𝑛  and  𝐗′𝑛  is  the  nearest  point  on  the  surface  of  the 
solid. 
𝑑 = ∣𝐗𝑛 − 𝐗′𝑛∣,
(30.6)
To  determine  𝐗′𝑛,  a  line  function  is  defined  which  passes  through  𝐗𝑛  and  is 
normal to the surface of the solid: 
Substituting the line function into the definition of the Equation (30.2) surface of a solid 
body gives: 
𝐋(𝑠) = 𝐗𝑛 + 𝑠𝐍 (𝐗𝑛).
(30.7)
LS-DYNA Theory Manual 
Geometric Contact Entities 
𝐺(𝐗𝑛 + 𝑠𝐍(𝐗)) = 0.
(30.8)
If  Equation  (30.8)  has  only  one  solution,  this  provides  the  parametric  coordinates  s 
which  locates  𝐗′𝑛.    If  Equation  (30.8)  has  more  than  one  root,  then  the  root  which 
minimizes Equation (30.6) locates the point 𝐗′𝑛. 
The penalty method defines the restoring forces as: 
𝐟 = 𝑝𝑑𝐍(𝐗′̅̅̅̅̅̅̅
𝑛),
(30.9)
where  𝑝  is  a  penalty  factor  and  is  effectively  a  spring  constant.    To  minimize  the 
penetration  of  the  slave  node  into  the  solid,  the  constant  𝑝  is  set  large,  however,  it 
should not be set so large that the Courant stability criteria is violated.  This criteria for 
the slave node tells us that: 
Δ𝑡 ≤
𝜔max
=
= 2√
𝑚𝑛
𝐾𝑛
, 
√𝐾𝑛
𝑚𝑛
(30.10)
where 𝐾𝑛 is the stiffness of node 𝑛 and 𝑚𝑛 is the mass of node 𝑛. 
The  penalty  factor,  𝑝,  is  determined  by  choosing  a  value  which  results  in  a 
penalty/slave mass oscillator which has a characteristic time step that is ten times larger 
than the Courant time step: 
Solving for 𝑝𝑛 gives: 
10Δ𝑡 = 2√
𝑚𝑛
𝑝𝑛
.
𝑝𝑛 =
4𝑚𝑛
(100Δ𝑡2)
.
(30.11)
(30.12)
Inclusion of any structural elements into the occupant model will typically result 
in  very  large  stiffnesses  due  to  the  small  time  step  and  the  (1/Δ𝑡)2  term.    Thus  the 
method is highly effective even with impact velocities on the order of 1km/sec. 
The  scalar  function  𝐺(𝐗)  is  frequently  more  conveniently  expressed  as 
𝑔(𝐱)where,  𝑔  is  the  function  defined  in  local  coordinates  and  𝐱  is  the  position  in  local 
coordinates.  The local entity is related to the global coordinates by: 
𝐱 = [T](𝐗𝑗 − 𝐐𝑗),
(30.13)
where  𝐐𝑗  is  the  offset  and  [T]  is  a  rotation  matrix.    The  solid  scalar  function  and  the 
penetration  distance  can  be  evaluated  in  either  local  or  global  coordinates  with  no 
difference  to  the  results.    When  working  in  local  coordinates,  the  gradient  of  the  local 
scalar  function  provides  a  normal  vector  which  is  in  the  local  system  and  must  be 
transformed into the global by:
Geometric Contact Entities 
LS-DYNA Theory Manual 
An ellipsoid is defined by the function: 
𝐍(𝐗̅̅̅̅̅) = [T]T𝐧(𝐱).
𝐺(𝑥, 𝑦, 𝑧) = (
)
+ (
)
+ (
)
− 1.
The gradient of 𝐺 is 2𝑥
𝑎2 𝐢 +
2𝑦
𝑎2 𝐣 + 2𝑧
𝐧(𝑥, 𝑦, 𝑧) =
𝑎2 𝐤 and the normal vector is: 
𝑏 2 𝐣 + 𝑧
𝑐 2 𝐤)
𝑦 2
𝑏 4 + 𝑧 2
( 𝑥
𝑎 2 𝐢 +
√𝑥 2
𝑎 4 +
𝑐 4
, 
Substituting Equations (30.7) and (30.15) into Equation (27.2) gives: 
[(
𝑛𝑥
𝑎  )
+ (
𝑛𝑦
𝑏  )
+ (
                            + [(
𝑛𝑧
𝑐  )
𝑥𝑛
] 𝑠 2 + 2 [
)
+ (
)
𝑦𝑛
𝑛𝑥𝑥𝑛
𝑎 2  +
𝑧𝑛
+ (
)
𝑛𝑦𝑦𝑛
𝑏 2  +
𝑛𝑧𝑧𝑛
𝑐 2  ] 𝑠  
− 1] = 0.
(30.14)
(30.15)
(30.16)
(30.17)
Solving this quadratic equation for 𝑠 provides the intercepts for the nearest point 
on the ellipsoid and the opposite point of the ellipsoid where the normal vector, 𝐗𝑛, also 
points toward.   
Currently, this method has been implemented for the case of an infinite plane, a 
cylinder,  a  sphere,  and  an  ellipsoid  with  appropriate  simplifications.    The  ellipsoid  is 
intended to be used with rigid body dummy models.  The methods are, however, quite 
general so that many more shapes could be  implemented.  A direct coupling to solids 
modeling packages should also be possible in the future.
LS-DYNA Theory Manual 
Nodal Constraints 
31    
Nodal Constraints 
In this section nodal constraints and linear constraint equations are described. 
31.1  Nodal Constraint Sets 
This  option  forces  groups  of  nodes  to  move  together  with  a  common 
translational  acceleration  in  either  one  or  more  degrees  of  freedom.    The  implementa-
tion is straightforward with the common acceleration defined by 
𝑎𝑖common =
𝑎𝑖
∑ 𝑀𝑗
∑ 𝑀𝑗
, 
(31.1)
where 𝑛 is the number of nodes, 𝑎𝑖
ith direction, and 𝑎𝑖common is the common acceleration.   
𝑗 is the acceleration of the jth constrained node in the 
Nodal constraint sets eliminate rigid body rotations in the body that contains the 
node set and, therefore, must be applied very cautiously. 
31.2  Linear Constraint Equations 
Linear constraint equations of the form: 
∑ 𝐶𝑘
𝑘=1
𝑢𝑘 = 𝐶0,
(31.2)
can  be  defined  where  𝑛  is  the  number  of  constrained  degrees  of  freedom,  𝑢𝑘  is  a 
constrained  nodal  displacement,  and  the  𝐶𝑘  are  user-defined  coefficients.    Unless  LS-
Nodal Constraints 
LS-DYNA Theory Manual 
DYNA  is  initialized  by  linking  to  an  implicit  code  to  satisfy  this  equation  at  the 
beginning  of  the  calculation,  the  constant  𝐶0  is  assumed  to  be  zero.    The  first 
constrained degree of freedom is eliminated from the equations of motion: 
𝑢1 = 𝐶0 − ∑
𝑘=2
𝐶𝑘
𝐶1
𝑢𝑘.
Its velocities and accelerations are given by 
𝑢̇1 = − ∑
𝑘=2
𝑢̈1 = − ∑
𝑘=2
𝐶𝑘
𝐶1
𝐶𝑘
𝐶1
𝑢̇𝑘,
𝑢̈𝑘
(31.3)
(31.4)
respectively.    In  the  implementation  a  transformation  matrix  𝐋  is  constructed  relating 
the  unconstrained  𝑢  and  constrained  𝑢constrained  degrees  of  freedom.    The  constrained 
accelerations used in the above equation are given by: 
𝑢constrained = [𝐋T𝐌𝐋]
−1
𝐋T𝐅,
(31.5)
where 𝐌 is the diagonal lumped mass matrix and 𝐅 is the righthand side force vector.  
This requires the inversion of the condensed mass matrix which is equal in size to the 
number  of  constrained  degrees  of  freedom  minus  one.    The  inverse  of  the  condensed 
mass matrix is computed in the initialization phase and stored in core.
LS-DYNA Theory Manual 
Vectorization and Parallelization 
32    
Vectorization and Parallelization 
32.1  Vectorization 
In  1978,  when  the  author  first  vectorized  DYNA3D  on  the  CRAY-1,  a  four-fold 
increase  in  speed  was  attained.    This  increase  was  realized  by  recoding  the  solution 
phase  to  process  vectors  in  place  of  scalars.    It  was  necessary  to  process  elements  in 
groups  rather  than  individually  as  had  been  done  earlier  on  the  CDC-7600 
supercomputers. 
Since vector registers are generally some multiple of 64 words, vector lengths of 
64 or some multiple are appropriate.  In LS-DYNA, groups of 128 elements or possibly 
some larger integer multiple of 64 are utilized.  Larger groups give a marginally faster 
code,  but  can  reduce  computer  time  sharing  efficiency  because  of  increased  core 
requirements.    If  elements  within  the  group  reference  more  than  one  material  model, 
subgroups  are  formed  for  consecutive  elements  that  reference  the  same  model.    LS-
DYNA internally sorts elements by material to maximize vector lengths. 
Conceptually,  vectorization  is  straightforward.    Each  scalar  operation  that  is 
normally executed once for one element, is repeated for each element in the group.  This 
means that each scalar is replaced by an array, and the operation is put into a DO-loop.  
For  example,  the  nodal  force  calculation  for  the  hexahedron  element  appeared  in  a 
scalar version of DYNA3D as: 
E11=SGV1*PX1+SGV4*PY1+SGV6*PZ1 
E21=SGV2*PY1+SGV4*PX1+SGV5*PZ1 
E31=SGV3*PZ1+SGV6*PX1+SGV5*PY1 
E12=SGV1*PX2+SGV4*PY2+SGV6*PZ2 
E22=SGV2*PY2+SGV4*PX2+SGV5*PZ2 
E32=SGV3*PZ2+SGV6*PX2+SGV5*PY2 
E13=SGV1*PX3+SGV4*PY3+SGV6*PZ3 
E23=SGV2*PY3+SGV4*PX3+SGV5*PZ3 
E33=SGV3*PZ3+SGV6*PX3+SGV5*PY3
Vectorization and Parallelization 
LS-DYNA Theory Manual 
E14=SGV1*PX4+SGV4*PY4+SGV6*PZ4 
E24=SGV2*PY4+SGV4*PX4+SGV5*PZ4 
E34=SGV3*PZ4+SGV6*PX4+SGV5*PY4 
and in the vectorized version as: 
DO 110 I = LFT, LLT 
E11(I)=SGV1(I)*PX1(I)+SGV4(I)*PY1(I)+SGV6(I)*PZ1(I) 
E21(I)=SGV2(I)*PY1(I)+SGV4(I)*PX1(I)+SGV5(I)*PZ1(I) 
E31(I)=SGV3(I)*PZ1(I)+SGV6(I)*PX1(I)+SGV5(I)*PY1(I) 
E12(I)=SGV1(I)*PX2(I)+SGV4(I)*PY2(I)+SGV6(I)*PZ2(I) 
E22(I)=SGV2(I)*PY2(I)+SGV4(I)*PX2(I)+SGV5(I)*PZ2(I) 
E32(I)=SGV3(I)*PZ2(I)+SGV6(I)*PX2(I)+SGV5(I)*PY2(I) 
E13(I)=SGV1(I)*PX3(I)+SGV4(I)*PY3(I)+SGV6(I)*PZ3(I) 
E23(I)=SGV2(I)*PY3(I)+SGV4(I)*PX3(I)+SGV5(I)*PZ3(I) 
E33(I)=SGV3(I)*PZ3(I)+SGV6(I)*PX3(I)+SGV5(I)*PY3(I) 
E14(I)=SGV1(I)*PX4(I)+SGV4(I)*PY4(I)+SGV6(I)*PZ4(I) 
E24(I)=SGV2(I)*PY4(I)+SGV4(I)*PX4(I)+SGV5(I)*PZ4(I) 
E34(I)=SGV3(I)*PZ4(I)+SGV6(I)*PX4(I)+SGV5(I)*PY4(I) 
110 
where 1 ≤ LFT ≤ LLT ≤ n.  Elements LFT to LLT inclusive use the same material model 
and n is an integer multiple of 64. 
Gather  operations  are  vectorized  on  most  supercomputers.    In  the  gather 
operation,  variables  needed  for  processing  the  element  group  are  pulled  from  global 
arrays into local vectors.  For example, the gather operation: 
DO 10 I 
X1(I) 
 =  
Y1(I) 
 =  
 =  
Z1(I) 
VX1(I)  =  
VY1(I)  =  
VZ1(I)  =  
 =  
X2(I) 
 =  
Y2(I) 
 =  
Z2(I) 
VX2(I)  =  
VY2(I)  =  
VZ2(I)  =  
 =  
X3(I) 
 =  
X3(I) 
 =  
X3(I) 
 =  
X8(I) 
 =  
Y8(I) 
Z8(I) 
 =  
VX8(I)  =  
LFT, LLT 
 =  
X(1,IX1(I)) 
X(2,IX1(I)) 
X(3,IX1(I)) 
V(1,IX1(I)) 
V(2,IX1(I)) 
V(3,IX1(I)) 
X(1,IX2(I)) 
X(2,IX2(I)) 
X(3,IX2(I)) 
V(1,IX2(I)) 
V(2,IX2(I)) 
V(3,IX2(I)) 
X(1,IX3(I)) 
X(2,IX3(I)) 
X(3,IX3(I)) 
X(1,IX8(I)) 
X(2,IX8(I)) 
X(3,IX8(I)) 
V(1,IX8(I))
LS-DYNA Theory Manual 
Vectorization and Parallelization 
VY8(I)  =  
VZ8(I)  =  
V(2,IX8(I)) 
V(3,IX8(I)) 
10 
initializes  the  nodal  velocity  and  coordinate  vector  for  each  element  in  the  subgroup 
LFT to LLT.  In the scatter operation, element nodal forces are added to the global force 
vector.  The force assembly does not vectorize unless special care is taken as described 
below. 
In general, the element force assembly is given in FORTRAN by: 
DO 30 I = 1,NODFRC 
DO 20 N = 1,NUMNOD 
DO 10 L = LFT,LLT 
RHS(I,IX(N,L))=RHS(I,IX(N,L))+FORCE(I,N,L) 
CONTINUE 
CONTINUE 
CONTINUE 
10 
20 
30 
where NODFRC is the number of force components per node (3 for solid elements, 6 for 
shells), LFT  and LLT  span the number of elements in the vector block,  NUMNOD is 
the number of nodes defining the element, FORCE contains the force components of the 
individual  elements,  and  RHS  is  the  global  force  vector.    This  loop  does  not  vectorize 
since the possibility exists that more that one element may contribute force to the same 
node.    FORTRAN  vector  compilers  recognize  this  and  will  vectorize  only  if  directives 
are added to the source code.  If all elements in the loop bounded by the limits LFT and 
LLT are disjoint, the compiler directives can be safely added.  We therefore attempt to 
sort the elements as shown in Figure 32.1 to guarantee disjointness. 
ELEMENT BLOCKING FOR VECTORIZATION
Vectorization and Parallelization 
LS-DYNA Theory Manual 
Block 1
Block 2
Block 3
Block 3
Figure 32.1.  Group of 48 elements broken into 4 disjoint blocks. 
The  current  implementation  was  strongly  motivated  by  Benson  [1989]  and  by 
work  performed  at  General  Motors  [Ginsberg  and  Johnson  1988, Ginsberg  and  Katnik 
1989], where it was shown that substantial improvements in execution speed could be 
realized by blocking the elements in the force assembly.  Katnik implemented element 
sorting  in  a  public  domain  version  of  DYNA3D  for  the  Belytschko-Tsay  shell  element 
and added compiler directives to force vectorization of the scatter operations associated 
with  the  addition  of  element  forces  into  the  global  force  vector.    The  sorting  was 
performed immediately after the elements were read in so that subsequent references to 
the stored element data were sequential.  Benson performed the sorting in the element 
loops via indirect addressing.  In LS-DYNA the published GM approach is taken. 
Implementation  of  the  vectorization  of the  scatter  operations  is  implemented  in 
for  all  elements  including  the  solid,  shell,  membrane,  beam,  and  truss  elements.    The 
sorting is completely transparent to the user. 
32.2  Parallelization 
In  parallelization,  the  biggest  hurdle 
is  overcoming  Amdahl’s 
law  for 
multitasking [Cray Research Inc.  1990] 
𝑆𝑚 =
𝑓𝑠 +
,
𝑓𝑝
(32.1)
where
LS-DYNA Theory Manual 
Vectorization and Parallelization 
𝑆𝑚 = maximum expected speedup from multitasking 
𝑁 = number of processors available for parallel execution 
𝑓𝑝 = fraction of a program that can execute in parallel 
𝑓𝑠 = fraction of a program that is serial 
Table  29.1  shows  that  to  obtain  a  speed  factor  of  four  on  eight  processors  it  is 
necessary to have eighty-six percent of the job running in parallel.  Obviously, to gain 
the highest speed factors the entire code must run in parallel. 
LS-DYNA  has  been  substantially  written  to  function  on  all  shared  memory 
parallel machine architectures.  Generally, shared memory parallel speed-ups of 5 on 8 
processors  are  possible  but  this  is  affected  by  the  machine  characteristics.    We  have 
observed speeds of 5.6 on full car crash models on a machine of one manufacturer only 
to see a speed-up of 3.5 on a different machine of another manufacturer. 
% 
N = 2  N = 4  N = 8  N = 16 N = 32 N = 64 N = 12
N = 256 
1.75 
86.0% 
1.82 
90.0% 
1.85 
92.0% 
1.89 
94.0% 
1.92 
96.0% 
1.96 
98.0% 
1.98 
99.0% 
1.98 
99.2% 
1.99 
99.4% 
1.99 
99.6% 
1.99 
99.7% 
2.00 
99.8% 
99.9% 
2.00 
100.0%  2.00 
2.82 
3.08 
3.23 
3.39 
3.57 
3.77 
3.88 
3.91 
39.3 
3.95 
3.96 
3.98 
3.99 
4.00 
4.04 
4.71 
5.13 
5.63 
6.25 
7.02 
7.48 
7.58 
7.68 
7.78 
7.84 
7.89 
7.94 
8.00 
5.16 
6.40 
7.27 
8.42 
10.00 
12.31 
13.91 
14.29 
14.68 
15.09 
15.31 
15.53 
15.76 
16.00 
5.99 
7.80 
9.20 
11.19 
14.29 
19.75 
24.43 
25.64 
26.98 
28.47 
29.28 
30.13 
31.04 
32.00 
6.52 
8.77 
10.60 
13.39 
18.18 
28.32 
39.26 
42.55 
46.44 
51.12 
53.83 
56.84 
60.21 
64.00 
8 
6.82 
9.34 
11.47 
14.85 
21.05 
36.16 
56.39 
63.49 
72.64 
84.88 
92.69 
102.07 
113.58 
128.00 
6.98 
9.66 
11.96 
15.71 
22.86 
41.97 
72.11 
84.21 
101.19 
126.73 
145.04 
169.54 
203.98 
256.00 
Table  29.1.Maximum  theoretical  speedup  Sm,  on  N  CPUs  with  parallelism  [Cray 
Research Inc.  1990]. 
In  the  element  loops  element  blocks  with  vector  lengths  of  64  or  some  multiple 
are assembled and  sent to separate processors.  All elements are processed in parallel.  
On  the  average  a  speed  factor  of  7.8  has  been  attained  in  each  element  class 
corresponding to 99.7% parallelization.   
A significant complication in parallelizing code is that a variable can sometimes 
be updated simultaneously by different processors with incorrect results.  To force the 
processors  to  access  and  update  the  variable  in  a  sequential  manner,  a  GUARD 
compiler  directive  must  be  introduced.    This  results  in  an  interruption  to  the  parallel
Vectorization and Parallelization 
LS-DYNA Theory Manual 
execution and can create a bottleneck.  By sorting the data in the parallel groups or by 
allocating  additional  storage  it  is  usually  possible  to  eradicate  the  GUARDS  from  the 
coding.  The effort may not be worth the gains in execution speed. 
The  element  blocks  are  defined  at  the  highest  level and  each  processor  updates 
the  entire  block  including  the  right  hand  side  force  assembly.    The  user  currently  has 
two  options:  GUARD  compiler  directives  prevent  simultaneous  updates  of  the  RHS 
vector  (recommended  for  single  CPU  processors  or  when  running  in  a  single  CPU 
mode  on  a  multi-processor),  or  assemble  the  right  hand  side  in  parallel  and  let  LS-
DYNA prevent conflicts between CPU’s.  This usually provides the highest speed and is 
recommended, i.e., no GUARDS.   
When executing LS-DYNA in parallel, the order of operations will vary from run 
to run.  This variation will lead to slightly different numerical results due to round-off 
errors.  By the time the calculation reaches completion variations in nodal accelerations 
and sometimes even velocities are observable.  These variations are independent of the 
precision and show up on both 32 and 64 bit machines.  There is an option in LS-DYNA 
to  use  an  ordered  summation  of  the  global  right  hand  side  force  vector  to  eliminate 
numerical  differences.    To  achieve  this  the  element  force  vectors  are  stored.    After 
leaving  the  element  loop,  the  global  force  vector  is  assembled  in  the  same  order  that 
occurs  on  one  processor.    The  ordered  summation  option  is  slower  and  uses  more 
memory than the default, but it leads to nearly identical, if not identical, results run to 
run.   
Parallelization in LS-DYNA was initially done with vector machines as the target 
where the vector speed up is typically 10 times faster than scalar.  On vector machines, 
therefore, vectorization comes first.  If the problem is large enough then parallelization 
is automatic.  If vector lengths are 128, for example, and if 256 beam elements are used 
only  a  factor  of  2  in  speed  can  be  anticipated  while  processing  beam  elements.    Large 
contact  surfaces  will  effectively  run  in  parallel,  small  surfaces  having  under  100 
segments will not.  The speed up in the contact subroutines has only registered 7 on 8 
processors  due  to  the  presence  of  GUARD  statements  around  the  force  assembly.  
Because  real  models  often  use  many  special  options  that  will  not  even  vectorize 
efficiently it is unlikely that more than 95% of a given problem will run in parallel on a 
shared memory parallel machine.
LS-DYNA Theory Manual 
Airbags 
33    
Airbags 
Additional 
information  on  the  airbag  modeling  and  comparisons  with 
experimental  data  can  be  found  in  a  report  [Hallquist,  Stillman,  Hughes,  and  Tarver 
1990]  based  on  research  sponsored  by  the  Motor  Vehicles  Manufacturers  Association 
(MVMA). 
33.1  Control Volume Modeling 
A direct approach for modeling the contents of the airbag would be to discretize 
the interior of the airbag using solid elements.  The total volume and pressure-volume 
relationship  of  the  airbag  would  then  be  the  sum  of  all  the  elemental  contributions.  
Although  this  direct  approach  could  be  applied  in  a  straight  forward  manner  to  an 
inflated airbag, it would become very difficult to implement during the inflation phase 
of  the  airbag  deployment.    Additionally,  as  the  model  is  refined,  the  solid  elements 
would  quickly  overwhelm  all  other  computational  costs  and  make  the  numerical 
simulations prohibitively expensive. 
An alternative approach for calculating the airbag volume, that is both applicable 
during  the  inflation  phase  and  less  computationally  demanding,  treats  the  airbag  as  a 
control volume.  The control volume is defined as the volume enclosed by a surface.  In 
the  present  case,  the  ‘control  surface’  that  defines  the  control  volume  is  the  surface 
modeled by shell or membrane elements comprising the airbag fabric material. 
Because  the  evolution  of  the  control  surface  is  known,  i.e.,  the  position, 
orientation,  and  current  surface  area  of  the  airbag  fabric  elements  are  computed  and 
stored  at  each  time  step,  we  can  take  advantage  of  these  properties  of  the  control 
surface elements to calculate the control volume, i.e., the airbag volume.  The area of the 
control surface can be related to the control volume through Green’s Theorem 
∭ 𝜙
∂𝜓
∂𝑥
𝑑𝑥𝑑𝑦𝑑𝑧 = − ∭ 𝜓
∂𝜙
∂𝑥
𝑑𝑥𝑑𝑦𝑑𝑧 + ∮ 𝜙𝜓𝑛𝑥𝑑𝛤 ,
(33.1)
Airbags 
LS-DYNA Theory Manual 
where  the  first  two  integrals  are  integrals  over  a  closed  volume,  i.e.,  𝑑𝑣 = 𝑑𝑥𝑑𝑦𝑑𝑧,  the 
last integral is an integral over the surface enclosing the volume, and 𝑛𝑥 is the direction 
cosine  between  the  surface  normal  and  the  𝑥  direction  (corresponding  to  the  x-partial 
derivative); similar forms can be written for the other two directions.  The two arbitrary 
functions 𝜙 and 𝜓 need only be integrated over the volume and surface. 
The integral form of the volume can be written as 
𝑉 = ∭ 𝑑𝑥𝑑𝑦𝑑𝑧.
(33.2)
Comparing the first of the volume integrals in Equation (33.1) to Equation (33.2), we can 
easily obtain the volume integral from Equation (33.1) by choosing for the two arbitrary 
functions 
𝜙 = 1,
𝜓 = 𝑥𝑥,
leading to 
𝑉 = ∫ ∫ ∫ 𝑑𝑥𝑑𝑦𝑑𝑧 = ∮ 𝑥𝑛𝑥𝑑𝛤 .
(33.3)
(33.4)
(33.5)
The surface integral in Equation (33.5) can be approximated by a summation over all the 
elements comprising the airbag, i.e., 
  ∮   𝑥𝑛𝑥𝑑𝛤 ≈ ∑ 𝑥̅𝑖𝑛𝑖𝑥𝐴𝑖
,
(33.6)
𝑖=1
where  for  each  element  i:  𝑥̅𝑖  is  the  average  x  coordinate,  𝑛𝑖𝑥  is  the  direction  cosine 
between  the  elements  normal  and  the  𝑥  direction,  and  𝐴𝑖  is  the  surface  area  of  the 
element. 
Although  Equation  (33.5)  will  provide  the  exact  analytical  volume  for  an 
arbitrary direction, i.e., any 𝑛, the numerical implementation of Equation (33.5), and its 
approximation  Equation  (33.6),  has  been  found  to  produce  slightly  different  volumes, 
differing  by  a  few  percent,  depending  on  the  choice  of  directions:    if  the  integration 
direction is nearly parallel to a surface element, i.e., the direction cosine is nearly zero, 
numerical  precision  errors  affect  the  volume  calculation.    The  implementation  uses  as 
an integration direction, a direction that is parallel to the maximum principle moment 
of inertia of the surface.  Numerical experiments have shown this choice of integration 
direction produces more accurate volumes than the coordinate or other principle inertia 
directions. 
Because airbag models may contain holes, e.g., holes for inflation and deflation, 
and Green’s Theorem only applies to closed surfaces, a special treatment is needed for 
calculating  the  volume  of  airbags  with  holes.    This  special  treatment  consists  of  the 
following:
LS-DYNA Theory Manual 
Airbags 
• 
The  n-sized  polygon  defining  the  hole  is  identified  automatically,  using 
edge locating algorithms in LS-DYNA. 
• 
The n-sized polygon is projected onto a plane, i.e., it is assumed to be flat; 
this  is  a  good  approximation  for  typical  airbag  hole  geometries.    Planar  symmetry 
should work with the control volume capability for one symmetry plane. 
• 
The area of the flat n-sided polygon is calculated using Green’s Theorem 
in two dimensions. 
• 
The resulting holes are processed as another surface element in the airbag 
control volume calculation. 
33.2  Equation of State Model 
As explained above, at each time step in the calculation the current volume of the 
airbag  is  determined  from  the  control  volume  calculation.    The  pressure  in  the  airbag 
corresponding to the control volume is determined from an equation of state (EOS) that 
relates the pressure to the current gas density (volume) and the specific internal energy 
of the gas. 
The  equation  of  state used  for  the  airbag  simulations  is  the  usual  ‘Gamma  Law 
Gas  
Equation of State’, 
𝑝 = (𝑘 − 1)𝜌𝑒,
(33.7)
where  𝑝  is  the  pressure,  𝑘  is  a  constant  defined  below,  𝜌  is  the  density,  and  𝑒  is  the 
specific internal energy of the gas.  The derivation of this equation of state is obtained 
from  thermodynamic  considerations  of  the  adiabatic  expansion  of  an  ideal  gas.    The 
incremental  change  in  internal  energy,  𝑑𝑈,  in  𝑛  moles  of  an  ideal  gas  due  to  an 
incremental increase in temperature, 𝑑𝑇, at constant volume is given by  
where 𝑐v is the specific heat at constant volume.  Using the ideal gas law we can relate 
the change in temperature to a change in the pressure and total volume, 𝑣, as 
𝑑𝑈 = 𝑛𝑐v𝑑𝑇,
(33.8)
𝑑(𝑝𝑣) = 𝑛𝑅𝑑𝑇,
(33.9)
where  𝑅  is  the  universal  gas  constant.    Solving  the  above  for  𝑑𝑇  and  substituting  the 
result into Equation (33.8) gives 
𝑑𝑈 =
𝑐v𝑑(𝑝𝑣)
=
𝑑(𝑝𝑣)
(𝑘 − 1)
,
where we have used the relationship 
𝑅 = 𝑐p − 𝑐v,
and the notation 
LS-DYNA Draft 
(33.10)
Airbags 
LS-DYNA Theory Manual 
Equation (33.10) may be rewritten as 
𝑘 =
𝑐p
𝑐v
.
and integrated to yield 
Solving for the pressure 
𝑑𝑈 =
𝜌0𝑣0
𝑘 − 1
𝑑 (
),
𝑒 =
𝜌0𝑣0
=
.
𝜌(𝑘 − 1)
𝑝 = (𝑘 − 1)𝜌𝑒.
(33.12)
(33.13)
(33.14)
(33.15)
The  equation  of  state  and  the  control  volume  calculation  can  only  be  used  to 
determine the pressure when the specific internal energy is also known.  The evolution 
equation for the internal energy is obtained by assuming the change in internal energy 
is given by 
𝑑𝑈 = −𝑝𝑑𝑣,
(33.16)
where the minus sign is introduced to emphasize that the volume increment is negative 
when  the  gas  is  being  compressed.    This  expression  can  be  written  in  terms  of  the 
specific internal energy as 
𝑑𝑒 =
𝑑𝑈
𝜌0𝑣0
= −
𝑝𝑑𝑣
𝜌0𝑣
.
Next, we divide the above by the equation of state, Equation (4.11.144), to obtain  
𝑑𝑒
= −
𝜌(𝑘 − 1)𝑑𝑣
𝜌0𝑣0
= −
(𝑘 − 1)𝑑𝑣
,
which may be integrated to yield 
ln𝑒 = (1 − 𝑘)ln𝑉,
or evaluating at two states and exponentiating both sides yields 
𝑒2 = 𝑒1 (
(1−𝑘)
)
.
𝑣2
𝑣1
(33.17)
(33.18)
(33.19)
(33.20)
The specific internal energy evolution equation, Equation (33.20), the equation of 
state,  Equation  (4.11.144),  and  the  control  volume  calculation  completely  define  the 
pressure-volume relation for an inflated airbag.
LS-DYNA Theory Manual 
Airbags 
33.3  Airbag Inflation Model 
Airbag  inflation  models  have  been  used  for many  years  in  occupant  simulation 
codes such as CAL3D [Fleck, 1981].   
The  inflation  model  we  chose  to  implement  in  LS-DYNA  is  due  to  Wang  and 
Nefske[1988] and more recent improvements to the model in LS-DYNA were suggested 
by Wang [1992].  In their development they consider the mass flow due to the vents and 
leakage through the bag.  We assume that the mass flow rate and the temperature of the 
gas going into the bag from an inflator are provided as tabulated functions of time.  
A pressure relation is defined: 
𝑄 =
𝑝e
𝑝2
,
(33.21)
where 𝑝e  is  the  external  pressure  and  𝑝2  is  the  internal  pressure  in  the  bag.    A  critical 
pressure relationship is defined as: 
𝑄crit = (
⁄
)
𝑘−1
,
𝑘 + 1
where 𝑘 is the ratio of specific heats: 
𝑘 =
𝑐p
𝑐v
.
If 𝑄 ≤ 𝑄crit then 𝑄 = 𝑄crit. 
Wang and Nefske define the mass flow through the vents and leakage by 
𝑚̇ 23 = 𝐶23𝐴23
𝑝2
𝑅√𝑇2
and 
𝑘⁄ √2𝑔𝑐 (
𝑘𝑅
𝑘 − 1
) (1 − 𝑄
𝑘−1
⁄ ),
𝑚̇ 23
′ = 𝐶′23𝐴′23
𝑝2
𝑅√𝑇2
𝑘⁄ √2𝑔𝑐 (
𝑘𝑅
𝑘 − 1
) (1 − 𝑄
𝑘−1
⁄ ),
(33.22)
(33.23)
(33.24)
(33.25)
where 𝐶23, 𝐴23, 𝐶′23, 𝐴′23, 𝑅 and 𝑔𝑐 are the vent orifice coefficient, vent orifice area, the 
orifice  coefficient  for  leakage,  the  area  for  leakage,  the  gas  constant,  and  the 
gravitational conversion constant, respectively.  The internal temperature of the airbag 
gas  is  denoted  by 𝑇2.   We  note  that  both 𝐴23  and  𝐴′23  can  be  defined  as  a  function  of 
pressure [Wang, 1992] or if they are input as zero they are computed within LS-DYNA.  
This latter option requires detailed modeling of the airbag with all holes included. 
A uniform temperature and pressure is assumed; therefore, in terms of the total 
airbag volume 𝑉2 and air mass, 𝑚2, the perfect gas law is applied:
Airbags 
LS-DYNA Theory Manual 
Solving for 𝑇2: 
𝑝2𝑉 = 𝑚2𝑅𝑇2.
(33.26)
𝑝2𝑉
𝑚2𝑅
and substituting Equation (33.27) into equations (33.25), we arrive at the mass transient 
equation: 
𝑇2 =
(33.27)
,
𝑚̇ out = 𝑚̇ 23 + 𝑚̇ 23
′ = 𝜇√2𝑝2𝜌
√
√
√
⎷
𝑘 − 𝑄
𝑘+1
⁄
)
𝑘 (𝑄
𝑘 − 1
(33.28)
where 
𝜌 = density of airbag gas, 
𝜇 = bag characterization parameter, 
𝑚̇ out = total mass flow rate out of bag. 
In terms of the constants used by Wang and Nefske: 
𝜇 = √𝑔𝑐(𝐶23𝐴23 + 𝐶′23𝐴′23).
(33.29)
We  solved  these  equations  iteratively,  via  function  evaluation.    Convergence  usually 
occurs in 2 to 3 iterations. 
The mass flow rate and gas temperature are defined in load curves as a function 
of time.  Using the mass flow rate we can easily compute the increase in internal energy: 
𝐸̇in = 𝑐p𝑚̇ in𝑇in,
(33.30)
where 𝑇in is the temperature of the gas flowing into the airbag.  Initializing the variables 
pressure,  𝑝,  density,  𝜌,  and  energy,  𝐸,  to  their  values  at  time  𝑛,  we  can  begin  the 
iterations loop to compute the new pressure, 𝑝𝑛 + 1, at time 𝑛 + 1. 
𝑝𝑛+1
2⁄ =
𝜌𝑛+1
2⁄ =
𝐸𝑛+1
2⁄ =
𝑝𝑛 + 𝑝𝑛+1
𝜌𝑛 + 𝜌𝑛+1
𝐸𝑛 + 𝐸𝑛+1
𝑄𝑛+1
2⁄ = max
⎜⎜⎜⎜⎛ 𝑝𝑒
𝑛+1
𝑝2
⎝
, 𝑄crit
. 
⎟⎟⎟⎟⎞
⎠
(33.31)
The mass flow rate out of the bag, 𝑚̇ out can now be computed: 
𝑛+1
𝑚̇ out
2⁄
33-6 (Airbags) 
= 𝜇√2𝑝2
𝑛+1
2⁄
√
√
√
√
⎷
𝜌𝑛+1
2⁄
⎜⎛𝑄𝑛+1
2⁄
⎝
𝑘⁄
− 𝑄𝑛+1
2⁄
𝑘+1
⁄
𝑘 − 1
⎟⎞
⎠
,
LS-DYNA Theory Manual 
Airbags 
where 
and the total mass updated: 
𝑛+1
𝑝2
2⁄
= 𝑝𝑛+1
2⁄ + 𝑝e,
𝑛+1
2⁄
𝑚𝑛+1 = 𝑚𝑛 + Δ𝑡 (𝑚̇ in
𝑚𝑛 + 𝑚𝑛+1
𝑚𝑛+1
2⁄ =
.
𝑛+1
− 𝑚out
2⁄
)
The energy exiting the airbag is given by: 
2⁄ 𝐸𝑛+1
2⁄
𝑚𝑛+1
2⁄
we can now compute our new energy at time 𝑛 + 1 
𝑛+1
= 𝑚̇ out
𝑛+1
out
2⁄
𝐸̇
,
𝐸𝑛+1 = 𝐸𝑛 + Δ𝑡 (Ė
2⁄
n+1
in
− 𝐸̇
2⁄
𝑛+1
out
) − 𝑝𝑛+1
2⁄ Δ𝑉𝑛+1
2⁄ ,
(33.33)
(33.34)
(33.35)
(33.36)
where Δ𝑉𝑛+1
be computed: 
2⁄  is the change in volume from time 𝑛 to 𝑛 + 1.  The new pressure can now 
𝑝𝑛+1 = (𝑘 − 1)
𝐸𝑛+1
𝑉𝑛+1,
(33.37)
which is the gamma-law (where 𝑘 = 𝛾) gas equation.  This ends the iteration loop. 
33.4  Wang's Hybrid Inflation Model 
Wang's proposed hybrid inflator model [1995a, 1995b] provides the basis for the 
model in LS-DYNA.  The first law of thermodynamics is used for an energy balance on 
the airbag control volume. 
𝑑𝑡
where 
(𝑚𝑢)cv = ∑ 𝑚̇ 𝑖 ℎ𝑖 − ∑ 𝑚̇ 𝑜 ℎ𝑜 − 𝑊̇ cv − 𝑄̇cv,
(33.38)
𝑑𝑡
(𝑚𝑢)cv =  rate of change of airbag internal energy 
∑ 𝑚𝑖 ℎ𝑖 =  energy into airbag by mass flow (e. g. , inflator) 
∑ 𝑚𝑜 ℎ𝑜 =  energy out of airbag by mass flow (e. g. , vents) 
𝑊̇ cv = ∫ 𝑃𝑑𝑉̇ =  work done by airbag expansion 
𝑄̇cv =  energy out by heat transfer through airbag surface.
Airbags 
LS-DYNA Theory Manual 
The rate of change of internal energy, the left hand side of Equation (33.38), can 
be differentiated: 
𝑑𝑡
𝑑𝑚
𝑑𝑡
where we have used the definition 
(𝑚𝑢) =
𝑑𝑚
𝑑𝑡
𝑢 + 𝑚
𝑑𝑢
𝑑𝑡
=
𝑢 + 𝑚
𝑑𝑡
(𝑐v𝑇) = 𝑚̇𝑢 + 𝑚𝑐 ̇v𝑇 + 𝑚𝑐v
𝑑𝑇
𝑑𝑡
, 
𝑢 = 𝑐v𝑇.
(33.39)
(33.40)
Then, the energy equation can be re-written for the rate of change in temperature 
for the airbag 
=
𝑑𝑇cv
𝑑𝑡
∑ 𝑚̇ 𝑖 ℎ𝑖 − ∑ 𝑚̇ 𝑜 ℎ𝑜 − 𝑊̇ cv − 𝑄̇cv − (𝑚̇𝑢)cv − (𝑚𝑐 ̇v𝑇)cv
(𝑚𝑐v)cv
Temperature  dependent  heat  capacities  are  used.    The  constant  pressure  molar  heat 
capacity is taken as: 
(33.41)
𝑐 ̅p = 𝑎 ̅ + 𝑏̅𝑇,
and the constant volume molar heat capacity as:  
𝑐 ̅v = 𝑎 ̅ + 𝑏̅𝑇 − 𝑟 ̅,
where 
𝑟 ̅ =  gas constant = 8.314 J/gm-mole K 
𝑎 ̅ =  constant [J/gm-mole K] 
𝑏̅ =  constant [J/gm-mole K2] 
(33.42)
(33.43)
Mass  based  values  are  obtained  by  dividing  the  molar  quantities  by  the 
molecular weight, 𝑀, of the gas 
𝑎 =
𝑎 ̅
,
𝑏 =
𝑏̅
,
𝑟 =
𝑟 ̅
.
The constant pressure and volume specific heats are then given by 
𝑐p = 𝑎 + 𝑏𝑇
𝑐v = 𝑎 + 𝑏𝑇 − 𝑟.
The specific enthalpy and internal energy becomes: 
ℎ = ∫ 𝑐𝑝𝑑𝑇
= 𝑎𝑇 +
𝑏𝑇2
𝑢 = ∫ 𝑐𝑣𝑑𝑇
= 𝑎𝑇 +
𝑏𝑇2
− 𝑟𝑇.
(33.44)
(33.45)
(33.46)
(33.47)
(33.48)
For ideal gas mixtures the molecular weight is given as:
LS-DYNA Theory Manual 
Airbags 
𝑀 =
,
∑
𝑓𝑖
𝑀𝑖
and the constant pressure and volume specific heats as: 
𝑐p = ∑ 𝑓𝑖 𝑐p(𝑖)
𝑐v = ∑ 𝑓𝑖 𝑐v(𝑖),
where 
𝑓𝑖 =  mass fraction of gas 𝑖 
𝑀𝑖 =  molecular weight of gas 𝑖 
𝑐p(𝑖) =  constant pressure specific heat of gas 𝑖 
𝑐v(𝑖) = constant volume specific heat of gas 𝑖. 
(33.49)
(33.50)
(33.51)
The  specific  enthalpy  and  internal  energy  for  an  ideal  gas  mixture  with 
temperature dependent heat capacity are 
ℎ = ∫ ∑ 𝑓𝑖
𝑐p(𝑖)𝑑𝑇 = ∑ 𝑓𝑖 (𝑎𝑖𝑇 +
𝑏𝑖𝑇2
)
𝑢 = ∫ ∑ 𝑓𝑖
𝑐v(𝑖)𝑑𝑇 = ∑ 𝑓𝑖 (𝑎𝑖𝑇 +
𝑏𝑖𝑇2
− 𝑟𝑖𝑇).
The rate of change of temperature for the airbag is 
𝑑𝑇cv
𝑑𝑡
=
∑ 𝑚̇ 𝑖 ℎ𝑖 − ∑ 𝑚̇ 𝑜 ℎ𝑜 − 𝑊̇ cv − 𝑄̇cv − (𝑚̇𝑢)cv − (𝑚𝑐 ̇v𝑇)cv
(𝑚𝑐v)cv
. 
The energy in by mass flow becomes: 
∑ 𝑚̇ 𝑖 ℎ𝑖 = ∑ 𝑚̇ 𝑖 (𝑎𝑖𝑇𝑖 +
𝑏𝑖𝑇𝑖
),
𝑚̇ 𝑖 is specified by an inflator mass inflow vs.  time table 
𝑇𝑖 is specified by an inflator temperature vs.  time table 
𝑎, 𝑏 are input constants for gas 𝑖 
And the energy out by mass flow: 
∑ 𝑚̇ 𝑜 ℎ𝑜 = ∑ 𝑚̇ 𝑜 [ ∑ 𝑓𝑖 (𝑎𝑖𝑇𝑐𝑣 +
gases
𝑏𝑖𝑇cv
)
].
(33.52)
(33.53)
(33.54)
(33.55)
(33.56)
The gas leaves the airbag at the control volume temperature 𝑇𝑐𝑣.  The mass flow 
rate  out  through  vents  and  fabric  leakage  is  calculated  by  the  one  dimensional
Airbags 
LS-DYNA Theory Manual 
isentropic  flow  equations  per  Wang  and  Nefske.    The  work  done  by  the  airbag 
expansion is given by: 
𝑊̇ cv = ∫ 𝑃𝑑𝑉̇ ,
(33.57)
𝑃 is calculated by the equation of state for a perfect gas, 𝑝 = 𝜌𝑅𝑇 and 𝑉̇  is calculated by 
LS-DYNA 
For the energy balance, we must compute the energy terms (𝑚̇ 𝑢)cv and (𝑚𝑐v)cv.  
Conservation of mass leads to: 
𝑚̇ cv = 𝑚̇ 𝑖 − 𝑚̇ 𝑜
𝑚cv = ∫ 𝑚̇ cv 𝑑𝑡.
The internal energy is given by  
𝑢cv = ∑ 𝑓𝑖 (𝑎𝑖𝑇cv +
𝑏𝑖𝑇cv
− 𝑟𝑖𝑇cv),
and the heat capacity at contact volume is: 
(𝑐v)cv = ∑ 𝑓𝑖 (𝑎𝑖 + 𝑏𝑖𝑇cv − 𝑟𝑖).
(33.58)
(33.59)
(33.60)
33.5  Constant Volume Tank Test 
Constant  volume  tank  tests  are  used  to  characterize  inflators.    The  inflator  is 
ignited  within  the  tank  and,  as  the  propellant  burns,  gas  is  generated.    The  inflator 
temperature is assumed to be constant.  From experimental measurements of the time 
history of the tank pressure it is straightforward to derive the mass flow rate, 𝑚̇ . From 
energy conservation, where 𝑇i and 𝑇t are defined to be the temperature of the inflator 
and tank, respectively, we obtain: 
𝑐p𝑚̇𝑇i = 𝑐v𝑚̇𝑇t + 𝑐v𝑚𝑇̇t.
For a perfect gas under constant volume, 𝑉̇ = 0, hence, 
𝑝̇𝑉 = 𝑚̇𝑅𝑇t + 𝑚𝑅𝑇̇t,
and, finally, we obtain the desired mass flow rate: 
𝑚̇ =
𝑐v𝑝̇𝑉
𝑐p𝑅𝑇i
.
(33.61)
(33.62)
(33.63)
LS-DYNA Theory Manual 
Dynamic Relaxation and System Damping 
34    
Dynamic Relaxation and System 
Damping 
Dynamic  relaxation  allows  LS-DYNA  to  approximate  solutions  to  linear  and 
nonlinear  static  or  quasi-static  processes.    Control  parameters  must  be  selected  with 
extreme  care  or  bad  results  can  be  obtained.    The  current  methods  are  not  compatible 
with  displacement  or  velocity  boundary  conditions,  but  various  body  loads,  thermal 
loads,  pressures,  and  nodal  loads  are  allowed.    The  solutions  to  most  nonlinear 
problems  are  path  dependent,  thus  results  obtained  in  the  presence  of  dynamic 
oscillations may not be the same as for a nonlinear implicit code, and they may diverge 
from reality. 
In  LS-DYNA  we  have  two  methods  of  damping  the  solution.    The  first  named 
“dynamic relaxation” is used in the beginning of the solution phase to obtain the initial 
stress  and  displacement  field  prior  to  beginning  the  analysis.    The  second  is  system 
damping which can be applied anytime during the solution phase either globally or on 
a material basis. 
34.1  Dynamic Relaxation For Initialization 
In  this  phase  only  a  subset  of  the  load  curves  is  used  to  apply  the  static  load 
which  is  flagged  in  the  load  curve  section  of  the  manual.    The  calculation  begins  and 
executes  like  a  normal  LS-DYNA  calculation  but  with  damping  incorporated  in  the 
update of the displacement field.  
Our  development  follows  the  work  of  Underwood  [1986]  and  Papadrakakis 
[1981] with the starting point being the dynamic equilibrium equation, Equation (23.1) 
with the addition of a damping term, at time 𝑛: 
𝐌𝐚𝑛 + 𝐂𝐯𝑛 + 𝐐𝑛(𝐝) = 0,
(34.1)
Dynamic Relaxation and System Damping 
LS-DYNA Theory Manual 
𝐐𝑛(𝐝) = 𝐅𝑛 − 𝐏𝑛 − 𝐇𝑛,
(34.2)
where we recall that 𝐌 is the mass matrix, 𝐂 is the damping matrix, 𝑛 indicates the nth 
time step, 𝐚𝑛 is the acceleration, 𝐯𝑛 the velocity, and 𝐝 is the displacement vector.  With 
Δ𝑡 as the fixed time increment we get for the central difference scheme: 
𝐯𝑛+1
2⁄ =
(𝐝𝑛+1 − 𝐝𝑛)
Δ𝑡
;
𝐚𝑛 =
For 𝐯𝑛 we can assume an averaged value 
(𝐯𝑛+1
2⁄ − 𝐯𝑛−1
Δ𝑡
2⁄ )
.
and obtain 
𝐯𝑛 =
(𝐯𝑛+1
2⁄ + 𝐯𝑛−1
2⁄ ),
𝐯𝑛+1
2⁄ = (
Δ𝑡
𝐌 +
−1
𝐂)
[(
Δ𝑡
𝐌 −
𝐂) 𝐯𝑛−1
2⁄ − 𝐐𝑛], 
𝐝𝑛+1 = 𝐝𝑛 + Δ𝑡𝐯𝑛+1
2⁄ .
(34.3)
(34.4)
(34.5)
(34.6)
In order to preserve the explicit form of the central difference integrator, 𝐌 and 
𝐂 must be diagonal.  For the dynamic relaxation scheme 𝐂 has the form 
If Equation (34.7) is substituted into (34.5) the following form is achieved 
𝐂 = 𝑐 ⋅ 𝐌.
𝐯𝑛+1
2⁄ =
2 − 𝑐Δ𝑡
2 + 𝑐Δ𝑡
𝐯𝑛−1
2⁄ +
2Δ𝑡
2 + 𝑐Δ𝑡
⋅ 𝐌−1 ⋅ 𝐐𝑛.
(34.7)
(34.8)
Since  𝐌  is  diagonal,  each  solution  vector  component  may  be  computed  individually 
from 
𝑛+1
𝐯𝑖
2⁄
=
2 − 𝑐Δ𝑡
2 + 𝑐Δ𝑡
𝑛−1
𝐯𝑖
2⁄
+
2Δ𝑡
2 + 𝑐Δ𝑡
𝐐𝑖
𝑚𝑖
.
As a starting procedure it is suggested by Underwood  
𝐯0 = 0
𝐝0 = 0.
(34.9)
(34.10)
Since the average value is used for 𝐯𝑛, which must be zero at the beginning for a quasi-
static solution 
thus the velocity at time +1 ⁄ 2 is 
𝐯−1
2⁄ = −𝐯
2⁄ ,
2⁄ = −
Δ𝑡
𝐌−1𝐐𝑜.
(34.11)
(34.12)
A damping coefficient must now be selected to obtain convergence to the static solution 
in minimal time.  The  best estimate for damping values is based on the frequencies of
LS-DYNA Theory Manual 
Dynamic Relaxation and System Damping 
the structure.  One choice is to focus on an optimal damping parameter as suggested by 
Papadrakakis  [1981].   Then  dynamic  relaxation  is  nothing else  but a  critically  damped 
dynamic system 
𝐶 = 𝐶cr = 2𝜔min𝑚,
(34.13)
with 𝑚 as modal mass.  The problem is finding the dominant eigenvalue in the structure 
related to the “pseudo-dynamic” behavior of the structure.  As the exact estimate would 
be  rather  costly  and  not  fit  into  the  explicit  algorithm,  an  estimate  must  be  used.  
Papadrakakis suggests 
𝜆𝐷 =
∥𝐝𝑛+1 − 𝐝𝑛∥
∥ 𝐝𝑛 − 𝐝𝑛−1∥
.
(34.14)
When  this  quantity  has  converged  to  an  almost  constant  value,  the  minimum 
eigenvalue of the structure can be estimated: 
2 = −
𝜔min
(𝜆𝐷
2 − 𝜆𝐷 ⋅ 𝛽 + 𝛼)
,
𝜆𝐷 ⋅ 𝛾
where 
𝛼 =
2 − 𝑐Δ𝑡
2 + 𝑐Δ𝑡
𝛽 = 𝛼 + 1 
2Δ𝑡2
2 + 𝑐Δ𝑡
𝛾 =
.
(34.15)
(34.16)
The  maximum  eigenvalue  determines  the time  step  and  is  already  known  from 
the model 
𝜔max
2 =
4.0
(Δ𝑡)2.
Now the automatic adjustment of the damping parameter closely follows the paper of 
Papadrakakis,  checking  the  current  convergence  rate  compared  to  the  optimal 
convergence  rate.    If  the  ratio  is  reasonably  close,  then  an  update  of  the  iteration 
parameters is performed. 
(34.17)
.
𝑐 =
4.0
Δ𝑡
√𝜔min
(𝜔min
⋅ 𝜔max
2 + 𝜔max
)
As is clearly visible from Equation (34.18) the value of highest frequency has always a 
rather  high  influence  on  the  damping  ratio.    This  results  in  a  non-optimal  damping 
ratio, if the solution is dominated by the response in a very low frequency compared to 
the  highest  frequency  of  the  structure.    This  is  typically  the  case  in  shell  structures, 
when bending dominates the solution.  It was our observation that the automatic choice 
following Papadrakakis results in very slow convergence for such structures, and this is 
also mentioned by Underwood for similar problems.  The damping ratio should then be 
fully  adjusted  to  the  lowest  frequency  by  hand  by  simply  choosing  a  rather  high 
(34.18)
Dynamic Relaxation and System Damping 
LS-DYNA Theory Manual 
damping  ratio.    An  automatic  adjustment  for  such  cases  is  under  preparation.    For 
structures with dominant frequencies rather close to the highest frequency, convergence 
is really improved with the automatically adjusted parameter. 
If the automated approach is not used then we apply the damping as 
𝐯𝑛+1
2⁄ = 𝜂𝐯𝑛−1
2⁄ + 𝐚𝑛Δ𝑡,
(34.19)
where 𝜂 is an input damping factor (defaulted to .995).  The factor, 𝜂, is equivalent to the 
corresponding factor in Equations (31.7- 31.8). 
The  relaxation  process  continues  until  a  convergence  criterion  based  on  the 
global kinetic energy is met, i.e., convergence is assumed if 
𝐸ke < CVTOL ⋅ 𝐸𝑘𝑒
max,
(34.20)
where  CVTOL  is  the  convergence  tolerance  (defaulted  to  .001).    The  kinetic  energy 
excludes any rigid body component.  Initial velocities assigned in the input are stored 
during  the  relaxation.    Once  convergence  is  attained  the  velocity  field  is  initialized  to 
the input values.  A termination time for the dynamic relaxation phase may be included 
in the input and is recommended since if convergence fails, LS-DYNA will continue to 
execute indefinitely. 
34.2  Mass Weighted Damping 
With mass weighted damping, the Equation (23.2) is modified as: 
𝐚𝑛 = 𝐌−1(𝐏𝑛 − 𝐅𝑛 + 𝐇𝑛 − 𝐅damp
),
where 
𝐹damp
= 𝐷𝑠𝑚𝑣.
(34.21)
(34.22)
As seen from Figure 34.1 and as discussed above the best damping constant for 
the system is usually the critical damping constant:  Therefore,  
𝐷𝑠 = 2𝜔min
(34.23)
is recommended. 
34.3  Dynamic Relaxation—How Fast Does it Converge?
LS-DYNA Theory Manual 
Dynamic Relaxation and System Damping 
The  number  of  cycles  required  to  reduce  the  amplitude  of  the  dynamic  response  by  a 
factor of 10 can be approximated by [see Stone, Krieg, and Beisinger 1985]  
ncycle = 1.15
𝜔max
𝜔min
.
(34.24)
Structural problems which involve shell and beam elements can have a very large ratio 
and 
consequently very slow convergence.
Figure  34.1.    Displacement  versus  time  curves  with  a  variety  of  damping
coefficients applied to a one degree-of-freedom oscillator.
LS-DYNA Theory Manual 
Heat Transfer 
35    
Heat Transfer 
LS-DYNA can be used to solve for the steady state or transient temperature field 
on  three-dimensional  geometries.    Material  properties  may  be  temperature  dependent 
and  either  isotropic  or  orthotropic.    A  variety  of  time  and  temperature  dependent 
boundary  conditions  can  be  specified  including  temperature,  flux,  convection,  and 
radiation.  The implementation of heat conduction into LS-DYNA is based on the work 
of Shapiro [1985]. 
35.1  Conduction of Heat in an Orthotropic Solid 
The  differential  equations  of  conduction  of  heat  in  a  three-dimensional 
continuum is given by 
𝜌𝑐𝑝
∂𝜃
∂𝑡
= (𝑘𝑖𝑗𝜃,𝑗)
,𝑖
+ 𝑄
(35.1)
subject  to  the  boundary  conditions,  𝜃 = 𝜃𝑠  on  Γ1,  𝑘𝑖𝑗𝜃,𝑗𝑛𝑖 + 𝛽𝜃 = 𝛾  on  Γ2,  and  initial 
conditions at 𝑡0: 
𝜃Γ = 𝜃0(𝑥𝑖) at   𝑡 = 𝑡0.
(35.2)
where 
𝜃 = 𝜃(𝑥𝑖, 𝑡)   temperature 
𝑥𝑖 = 𝑥𝑖(𝑡)   coordinates as a function of time 
𝜌 = 𝜌(𝑥𝑖)   density 
𝑐𝑝 = 𝑐𝑝(𝑥𝑖, 𝜃)   specific heat capacity 
𝑘𝑖𝑗 = 𝑘𝑖𝑗(𝑥𝑖, 𝜃)   thermal conductivity 
𝑄 = 𝑄(𝑥𝑖, 𝜃)   internal heat generation rate per unit volume Ω 
𝜃Γ =  prescribed temperature on Γ1 
𝑛𝑖 = normal vector to  Γ2 
Equations  (35.1)-(35.2)  represent  the  strong  form  of  a  boundary  value  problem  to  be 
solved for the temperature field within the solid.
Heat Transfer 
LS-DYNA Theory Manual 
DYNA3D  employs  essentially  the  same  theory  as  TOPAZ  [Shapiro  1985]  in 
solving  Equation  (35.1)  by  the  finite  element  method.    Those  interested  in  a  more 
detailed  description  of  the  theory  are  referred  to  the  TOPAZ  User’s  Manual.    Brick 
elements  are  integrated  with  a  2 × 2 × 2  Gauss  quadrature  rule,  with  temperature 
dependence  of  the  properties  accounted  for  at  the  Gauss  points.    Time  integration  is 
performed  using  a  generalized  trapezoidal  method  shown  by  Hughes  to  be 
unconditionally  stable  for  nonlinear  problems.    Newton’s  method  is  used  to  satisfy 
equilibrium in nonlinear problems. 
The  finite  element  method  provides  the  following  equations  for  the  numerical 
solution of Equations (35.1)-(35.2) 
[
𝐶𝑛+𝛼
Δ𝑡
+ 𝛼𝐻𝑛+𝛼] {𝜃𝑛+1 − 𝜃𝑛} = {𝐹𝑛+𝛼 − 𝐻𝑛+𝛼𝜃𝑛}
where  
𝑒 ]
[𝐶] = ∑[𝐶𝑖𝑗
= ∑ ∫ 𝑁𝑖𝜌𝑐𝑁𝑗𝑑Ω
Ω𝑒
𝑒 ]
[𝐻] = ∑[𝐻𝑖𝑗
= ∑
⎢⎡ ∫ ∇𝑇𝑁𝑖𝐾∇𝑁𝑗𝑑Ω + ∫ 𝑁𝑖𝛽𝑁𝑗𝑑Γ
⎣
Ω𝑒
Γ𝑒
⎥⎤
⎦
𝑒]
[𝐹] = ∑[𝐹𝑖
= ∑
⎢⎡ ∫ 𝑁𝑖𝑞𝑔𝑑Ω + ∫ 𝑁𝑖𝛾𝑑Γ
⎣
Ω𝑒
Γ𝑒
⎥⎤
⎦
(35.3)
(35.4)
(35.5)
(35.6)
The parameter 𝛼 is taken to be in the interval [0,1].  Some well-known members 
of this 𝛼-family are 
•𝛼 Method 
•  0 
forward difference; forward Euler 
•  1⁄2  midpoint rule; Crank-Nicolson 
•  2⁄3  Galerkin 
•  1 
backward difference, fully implicit 
35.2  Thermal Boundary Conditions 
Boundary conditions are represented by
LS-DYNA Theory Manual 
Heat Transfer 
𝑘𝑥
∂𝜃
∂𝑥
𝑛𝑥 + 𝑘𝑦
∂𝜃
∂𝑦
𝑛𝑦 + 𝑘𝑧
∂𝜃
∂𝑧
𝑛𝑧 = 𝛾 − 𝛽𝜃 = 𝑞′′̇ .
(35.7)
By  convention,  heat  flow  is  positive  in  the  direction  of  the  surface  outward  normal 
vector.    Surface  definition  is  in  accordance  with  the  right  hand  rule.    The  outward 
normal  vector  points  to  the  right  as  one  progresses  from  node  N1  to  N2  to  N3  and 
finally to N4.  See Figure 35.1. 
Boundary  conditions  can  be  functions  of  temperature  or  time.    More  than  one 
boundary  condition  can  be  specified  over  the  same  surface  such  as  in  a  case  of 
combined  convection  and  radiation.    For  situations  where  it  is  desired  to  specify 
adiabatic  (i.e.,  𝑞′′̇ = 0)  conditions,  such  as  at  an  insulated  surface  or  on  a  line  of 
symmetry,  no  boundary  condition  need  be  specified.    This  is  the  default  boundary 
condition in LS-DYNA. 
Temperature  boundary  condition  can  be  specified  on  any  node  whether  on  the 
physical boundary or not. 
Flux,  convection,  and  radiation  boundary  conditions  are  specified  on  element 
surface  segments  defined  by  3  (triangular  surface)  or  4  nodes  (quadrilateral  surface).  
These  boundary  conditions  can  be  specified  on  any  finite  element  surface  whether  on 
the physical boundary or not.  
•  Flux:    Set  𝑞′′̇ = 𝑞𝑓 ,  where  𝑞𝑓   is  defined  at  the  node  points  comprising  the  flux 
boundary condition surface.  
•  Convection:  A  convection  boundary  condition  is  calculated  using  𝑞′′̇ = ℎ(𝑇 −
𝑇∞), where ℎ is heat transfer coefficient, (𝑇 − 𝑇∞) is temperature potential.  LS-
DYNA evaluates ℎ at the film temperature 
N1
N4
N3
N2
Figure 35.1.  Definition of the outward normal vector
Heat Transfer 
LS-DYNA Theory Manual 
𝑇 =
(𝑇surf + 𝑇∞)
(35.8)
•  Radiation:    A  radiation  boundary  condition  is  calculated  using  𝑞′′̇ = ℎ 𝑟(𝑇4 −
4 ), where ℎ 𝑟 = 𝜎𝜀𝐹 is a radiant-heat-transfer coefficient.  
𝑇∞
35.3  Thermal Energy Balances 
Various  energy  terms  are  printed  and  written  into  the  plot  file  for  post 
processing using the code LS-PREPOST.  The energy terms are: 
• 
• 
• 
• 
• 
change in material internal energy for time step, 
change in material internal energy from initial time, 
heat transfer rates on boundary condition surfaces, 
heat transfer rates on enclosure radiation surfaces, 
𝑥, 𝑦, and 𝑧 fluxes at all nodes. 
35.4  Heat Generation 
Volumetric  heat  generation  rates  may  be  specified  by  element,  by  material,  or 
both  (in  which  case  the  effect  is  additive).    Volumetric  heat  generation  rates  can  be  a 
function of time or temperature. 
35.5  Initial Conditions 
Initial temperature conditions can be  specified on the nodal data input cards or 
on the nodal temperature initial condition cards.  If no temperatures are specified, the 
default  is  0.    For  nonlinear  steady  state  problems  the  temperature  initial  condition 
serves as a first guess for the equilibrium iterations. 
35.6  Material Properties 
Heat capacity and thermal conductivity may be functions of temperature.  Since 
the density and heat capacity appear only as a product in the governing equations, the
LS-DYNA Theory Manual 
Heat Transfer 
temperature  dependence  of  the  density  may  be  included  in  the  temperature 
dependence  of  the  heat  capacity.    Material  properties  are  evaluated  at  the  element 
Gauss point temperature or average element temperature. 
The  thermal  conductivity  may  be  either  isotropic  or  orthotropic.    For  an 
orthotropic  material,  the  three  material  axes  (𝑥′1, 𝑥′2, 𝑥′3)  are  orthogonal  and  the 
thermal conductivity tensor 𝐊 is diagonal. 
The thermal conductivity tensor 𝐊 in the global coordinate system is related by 
where 
𝐾𝑖𝑗 = 𝐾′𝑖𝑗𝛽𝑚𝑖𝛽𝑛𝑗,
𝛽𝑖𝑗 = cos(𝑥′𝑖, 𝑥𝑗).
(35.9)
(35.10)
35.7  Nonlinear Analysis 
In  a  nonlinear  problem,  𝐶,  𝐻,  and  𝐹  are  functions  of  temperature.  Newton’s 
method  is  used  to  transform  equation  32.4  into  an  alternate  form  which  contains 
temperature derivatives of 𝐶, 𝐻, and 𝐹 (i.e., the tangent matrix).  Iterations are required 
to solve this alternate form. 
In a steady state nonlinear problem, an initial guess should be made of the final 
temperature  distribution  and  included  in  the  input  file  as  an  initial  condition.   If  your 
guess is good, a considerable savings in computation time is achieved. 
35.8  Units 
Any consistent set of units with the governing equation may be used.  Examples 
are: 
Quantity 
temperature 
space 
time 
density 
heat capacity 
thermal conductivity 
thermal generation 
Units 
K 
m 
s 
kg/m3 
J/kg k 
W/m K 
W/M3 
F 
C 
ft 
cm 
hr 
s 
Lbm/ft3 
g/cm3 
cal/g c 
Btu/LbmF 
cal/s cm C  Btu/hr ft F 
Btu/hr ft3 
cal/s cm3
Heat Transfer 
LS-DYNA Theory Manual 
heat flux 
W/m2 
cal/s cm2 
Btu/hr ft2
LS-DYNA Theory Manual 
Adaptivity 
36    
Adaptivity 
LS-DYNA  includes  an  h-adaptive  method  for  the  shell  elements.    In  an 
h-adaptive  method,  the  elements  are  subdivided  into  smaller  elements  wherever  an 
error indicator shows that subdivision of the elements will provide improved accuracy.  
An  example  of  an  adaptive  calculation  on  a  thin  wall  square  cross  section  beam  is 
shown in Figure 36.1.  In Figures 36.2 through 36.4 a simple metal stamping simulation 
is  shown  [also  see  Galbraith,  Finn,  et.    al.,  1991].    In  the  following,  the  methodologies 
used  in  the  h-adaptive  method  in  LS-DYNA  are  described.    The  objective  of  the 
adaptive process used in LS-DYNA is to obtain the greatest accuracy for a given set of 
computational  resources.    The  user  sets  the  initial  mesh  and  the  maximum  level  of 
adaptivity,  and  the  program  subdivides  those  elements  in which  the  error  indicator  is 
the largest.  Although this does not provide control on the error of the solution, it makes 
it possible to obtain a solution of comparable accuracy with fewer elements, and, hence, 
less computational resources, than with a fixed mesh. 
LS-DYNA  uses  an  h-adaptive  process,  where  parts  of  the  mesh  are  selectively 
refined during the course of the solution procedure.  The methodology used is based on 
Belytschko,  Wong,  and  Plaskacz  [1989].    In  the  former,  elements  were  also  fused  or 
combined  when  it  was  felt  that  they  were  no  longer  needed.    It  was  found  that  the 
implementation  of  fusing  procedures  for  general  meshes,  such  as  occur  in  typical 
applications  of  commercial  programs,  is  too  complex,  so  only  fission  is  included.  
Adaptivity in LS-DYNA can be restricted to specific groups of shell elements.  Elements 
that fall in this group are said to be in the active adaptivity domain.
Adaptivity 
LS-DYNA Theory Manual 
  Figure 36.1.  One level adaptive calculation on a square cross section beam. 
  Figure 36.2.  Aluminum blank with 400 shells in blank and four rigid tools.
LS-DYNA Theory Manual 
Adaptivity 
Figure 36.3.  Adaptive calculations using two adaptive levels. 
In the h-adaptive process, elements are subdivided into smaller elements where 
more  accuracy  is  needed;  this  process  is  called  fission.    The  elements  involved  in  the 
fission process are subdivided into elements with sides ℎ/2, where ℎ is the characteristic 
size  of  the  original  elements.    This  is  illustrated  in  Figure  36.5  for  a  quadrilateral 
element.    In  fission,  each  quadrilateral  is  subdivided  into  four  quadrilaterals  (as 
indicated  in  Figure  36.2)  by  using  the  mid-points  of  the  sides  and  the  centroid  of  the 
element to generate four new quadrilaterals.  
  Figure 36.4.  Final shape of formed part with 4315 shell elements per quarter.
Adaptivity 
LS-DYNA Theory Manual 
Figure 36.5.  Fissioning of a Quadrilateral Element 
The  fission  process  for  a  triangular  element  is  shown  in  Figure  36.6  where  the 
element  is  subdivided  into  four  triangles  by  using  the  mid-points  of  the  three  sides.  
The  adaptive  process  can  consist  of  several  levels  of  fission.    Figure 36.5  shows  one 
subdivision,  which  is  called  the  second  refinement  level.    In  subsequent  steps,  the 
fissioned elements can again be fissioned in a third refinement level, and these elements 
can again, in turn, be fissioned in a fourth level, as shown in Figure 36.7.  The levels of 
adaptivity that occur in a mesh are restricted by three rules: 
•  The  number  of  levels  is  restricted  by  the  maximum  level  of  adaptivity  that  is 
allowed in the mesh, which is generally set at 3 or 4.  At the fourth level up to 64 
elements will be generated for each element in the initial mesh. 
•  The levels of adaptivity implemented in a mesh must be  such that the levels of 
adaptivity implemented in adjacent elements differ by, at most, one level. 
•  The  total  number  of  elements  can  be  restricted  by  available  memory.   Once the 
specified memory usage is reached, adaptivity ceases. 
The  second  rule  is  used  to  enforce  a  2-to-1  rule  given  by  Oden,  Devloo  and 
Strouboulis [1986], which restricts the number of elements along the side of any element 
in  the  mesh  to  two.    The  enforcement  of  this  rule  is  necessary  to  accommodate 
limitations in the data structure.   
The  original  mesh  provided  by  the  user  is  known  as  the  parent  mesh,  the 
elements  of  this  mesh  are  called  the  parent  elements,  and  the  nodes  are  called  parent 
Figure 36.6.  Fissioning of a Triangular Element 
nodes.  Any elements that are generated by the adaptive process are called descendant
LS-DYNA Theory Manual 
Adaptivity 
Figure 36.7.  Quadrilateral Element Fissioned to the fourth level 
elements,  and  any  nodes  that  are  generated  by  the  adaptive  process  are  called 
descendant nodes.  Elements generated by the second level of adaptivity are called first-
generation  elements,  those  generated  by  third  level  of  adaptivity  are  called  second-
generation elements, etc. 
The  coordinates  of  the  descendant  nodes  are  generated  by  using  linear 
interpolation.  Thus, the coordinates of any node generated during fission of an element 
are given by 
𝑥𝑁 =
(𝑥𝐼 + 𝑥𝐽),
(36.1)
where  𝑥𝑁  is  the  position  of  the  generated  node  and  𝑥𝐼  and  𝑥𝐽  are  the  nodes  along  the 
side  on  which  𝑥𝑁  was  generated  for  a  typical  element  as  shown  in  Fig. 33.1.    The 
coordinate  of  the  mid-point  node,  which  is  generated  by  fission  of  a  quadrilateral 
element, is given by 
𝑥𝑀 =
(𝑥𝐼 + 𝑥𝐽 + 𝑥𝐾 + 𝑥𝐿),
(36.2)
where 𝑥𝑀 is the new midpoint node of the fissioned quadrilateral and 𝑥𝐼, 𝑥𝐽, 𝑥𝐾 and 𝑥𝐿 
are the nodes of the original quadrilateral.  The velocities of the nodes are also given by 
linear interpolation.  The velocities of edge nodes are given by  
and the angular velocities are given by 
𝑣𝑁 =
(𝑣𝐼 + 𝑣𝐽),
𝜔𝑁 =
(𝜔𝐼 + 𝜔𝐽).
The velocities of a mid-point node of a fissioned quadrilateral element are given by 
𝑣𝑀 =
(𝑣𝐼 + 𝑣𝐽 + 𝑣𝐾 + 𝑣𝐿),
𝜔𝑀 =
(𝜔𝐼 + 𝜔𝐽 + 𝜔𝐾 + 𝜔𝐿).
(36.3)
(36.4)
(36.5)
(36.6)
Adaptivity 
LS-DYNA Theory Manual 
out-of-plane
undeformed
deformed
Figure 36.8.  Refinement indicator based on angle change. 
The stresses in the descendant element are obtained from the parent element by 
setting  the  stresses  in  the  descendant  elements  equal  to  the  stresses  in  the  parent 
element at the corresponding through-the-thickness quadrature points. 
In  subsequent  steps,  nodes  which  are  not  corner  nodes  of  an  all  attached 
elements  are  treated  as  slave  nodes.    They  are  handled  by  the  simple  constraint 
equation. 
Refinement indicators are used to decide the locations of mesh refinement.  One 
deformation  based  approach  checks  for  a  change  in  angles  between  contiguous 
elements as shown in Figure 36.8.  If  𝜁 > 𝜁tol then refinement is indicated, where 𝜁tol is 
user defined.
LS-DYNA Theory Manual 
Adaptivity 
Figure  36.9.    The  input  parameter,  ADPASS,  controls  whether  LS-DYNA 
backs up and repeats the calculation after adaptive refinement. 
After  the  mesh  refinement  is  determined,  we  can  refine  the  mesh  and  continue 
the calculation or back up to an earlier time and repeat part of the calculation with the 
new mesh.  For accuracy and stability reasons the latter method is generally preferred; 
however, the former method is preferred for speed.  Whether LS-DYNA backs up and 
repeats  the  calculation  or  continues  after  remeshing  is  determined  by  an  input 
parameter, ADPASS.  This is illustrated in Figure 36.9.
LS-DYNA Theory Manual 
Implicit 
37    
Implicit 
37.1  Introduction 
Implicit solvers are properly applied to static, quasi-static, and dynamic problems with 
a low frequency content.  Such applications include but are not limited to 
•  Static and quasi-static structural design and analysis 
•  Metal forming, especially, the binderwrap and springback 
•  Gravitational loading of automotive structures 
•  Linear buckling and vibration analysis 
An advantage of the implicit solver on explicit integration is that the number of load or 
time steps is typically 100 to 10000 times fewer.  The major disadvantage is that the cost 
per  step  is  unknown  since  the  speed  depends  mostly  on  the  convergence  behavior  of 
the equilibrium iterations which can vary widely from problem to problem.   
An  incremental-iterative  numerical  algorithm  is  implemented  in  LS-DYNA.    The 
method  is  stable  for  wide  range  of  nonlinear  problems  that  involve  finite  strain  and 
arbitrarily large rotations.  Accuracy consideration usually limits the load increment or 
time step size.  An inaccurate solution will often not converge.  Nine iterative schemes 
are  available  including  the  full  Newton  method  and  eight  quasi-Newton  methods.  
These are: 
•  Full Newton, 
•  BFGS (default), 
•  Broyden, 
•  Davidon-Fletcher-Powell (DFP) [Schweizerhof 1986], 
•  Davidon symmetric, [Schweizerhof 1986], 
•  modified constant arc length with BFGS,
Implicit 
LS-DYNA Theory Manual 
•  modified constant arc length with Broyden’s, 
•  modified constant arc length with DFP, 
•  modified constant arc length with Davidon. 
A  line  search  is  combined  with  each  of  these  schemes  along  with  automatic  stiffness 
reformations,  as  needed,  to  avoid  non-convergence.    LS-DYNA  defaults  to  the  BFGS 
quasi-Newton  method  which  is  the  most  robust  although  the  other  methods  are 
sometimes  superior.    Generally,  the  quasi-Newton  methods  require  fewer  iterations 
than the modified Newton method since they exhibit superlinear local convergence due 
to the rank one or rank two updates of the stiffness matrix as the iterations proceed.  In 
this  chapter,  important  aspects  of  the  static  and  dynamic  algorithm  are  explained, 
hopefully, in a way that will be understandable to all users.  The arc length methods are 
generally  used  in  solving  snap  through  buckling  problems  and  details  on  one  specific 
implementation is taken up in the next chapter. 
37.2  Equations 
37.2.1  Discretization 
Neglecting constraints, discretization formally leads to the matrix equations of motion 
𝑹 = 𝑴𝒙̈ + 𝑭𝑖 − 𝑭𝑒 = 𝟎
(37.1)
where 
𝒙̈ = acceleration vector of length 𝑛 
𝑴 = 𝑛 × 𝑛 mass matrix 
𝑭𝑒 = body force and external load vector of length 𝑛 
𝑭𝑖 = internal force vector of length 𝑛. 
It is implicitly assumed that the involved vectors 𝑭𝑖 and 𝑭𝑒 depend on6 
𝒙̇, 𝒙 =  velocity and coordinate vectors of length 𝑛 
𝑡 = simulation time 
as well as on some history of the deformation, while 𝑴 is constant.  In practice, the only 
independent variable is 𝒙 since the velocity 𝒙̇ and acceleration 𝒙̈ are typically expressed 
in terms of this coordinate vector by the time integration scheme  used, and  𝑡 is given.  
Deformation  history  is  typically  accounted  for  in  internal  variables  associated  with 
features  in  the  model,  such  as  plastic  strains  in  materials  and  frictional  sliding  in 
contacts. 
6 This is true prior to time discretization, vectors 𝑭(cid:3036) and 𝑭(cid:3032) depend on 𝒙 and on 𝒙(cid:4662)  only through the exact 
time differentiation. Once time discretization is done according to some scheme, the dependence is on 𝒙 
and not necessarily on the discretized 𝒙(cid:4662)  but rather ∆𝒙/∆𝑡, see Section 1.4.1.
LS-DYNA Theory Manual 
Implicit 
A diagonal lumped mass matrix is obtained by row summing according to  
𝑀𝑖𝑖 = ∫ 𝜌𝜙𝑖 ∑ 𝜙𝑗
𝑑𝑉
= ∫ 𝜌𝜙𝑖𝑑𝑉
(37.2)
where 𝜌 is material density and 𝑉 denotes the body over which integration occurs. 
The  primary  nonlinearities,  which  are  due  to  geometric  effects  and  inelastic  material 
behavior, are accounted for in 𝑭𝑖, 
𝑭𝑖 = ∫ 𝑩𝑇𝝈𝑑𝑉
,
(37.3)
where 𝑩 is the strain-displacement matrix and 𝝈 is the stress. 
Additional nonlinearities arise in 𝑭𝑒 due to geometry dependent applied loads, such as 
contacts and loads on segments. 
Explicit  integration  trivially  satisfies  (37.1)  since  the  calculation  of  the  acceleration 
guarantees equilibrium, i.e., from time step 𝑗 to 𝑗 + 1 we use 
𝒙̈𝑗 = 𝑴 −1[𝑭𝑒
𝑗 − 𝑭𝑖
𝑗].
The explicit update of the velocities and coordinates is given by 
𝒙̇ 𝑗+1/2 = 𝒙̇ 𝑗−1/2 + 𝛥𝑡𝑗𝒙̈𝑗,
𝒙𝑗+1 = 𝒙𝑗 + 𝛥𝑡𝑗+1/2𝒙̇𝑗+1/2.
(37.4)
(37.5)
(37.6)
Stability  places  a  limit  on  the  time  size.    This  step  size  may  be  very  small  and, 
consequently,  a  large  number  of  steps  may  be  required.    Implicit  analysis  employs 
schemes  that  are  unconditionally  stable,  thus  allowing  for  larger  steps  at  the  cost  of  a 
more expensive update of the geometry. 
37.2.2  Constraints 
Constraints is obviously an important ingredient in nonlinear finite elements, and may 
include for instance simple point or motion constraints, slave nodes constrained to rigid 
bodies, joints and tied contacts.  Constraints are divided into two categories, those that 
are  directly  eliminated  (first  kind)  and  those  that  are  treated  with  Lagrangian 
multipliers 𝝀 (second kind).  The principle behind (37.1) is that of virtual work, stating 
that 
𝛿𝒙𝑇(𝑹 + 𝑪𝜆
𝑇𝝀) = 0
(37.7)
for  any  admissible  virtual  displacement  field  𝛿𝒙.  Admissible  displacement  fields  are 
those that satisfy the first kind of constraints.  The second kind is instead treated by the
Implicit 
LS-DYNA Theory Manual 
second  term  inside  the  parenthesis,  for  which  we  require  satisfaction  of  𝑚𝜆  additional 
constraints 
𝑯𝜆(𝒙, 𝑡) = 𝟎
(37.8)
and 
𝜕𝑯𝜆
𝜕𝒙
If  there  are  no  constraint  of  the  first  kind,  any  displacement  field  is  admissible  and 
𝑇𝝀 = 𝟎. The presence of first kind constraints put restrictions on 𝛿𝒙 and the 
hence 𝑹 + 𝑪𝜆
following is an attempt to derive the proper nonlinear equations in this context. 
𝑪𝜆 =
(37.9)
.
Constraints  of  the  first  kind  augment  the  𝑛  equations  of  motion  by  imposing  𝑚 
additional equations 
and consequently (37.1) is to be reduced to 𝑛 − 𝑚 equations.  To this end, we introduce 
the 𝑚 × 𝑛 constraint matrix 
𝑯(𝒙, 𝑡) = 𝟎,
(37.10)
𝑪 =
𝜕𝑯
𝜕𝒙
,
(37.11)
and conveniently partition the global vector 𝒙 into an independent (solution) part 𝒙𝐼 of 
length  𝑛 − 𝑚  and  dependent  part  𝒙𝐷  of  length  𝑚.  This  partitioning  is  represented  by 
projection matrices 𝑷𝐼 and 𝑷𝐷 such that 
and 
𝒙𝐼 = 𝑷𝐼𝒙,
𝒙𝐷 = 𝑷𝐷𝒙
𝒙 = 𝑷𝐼
𝑇𝒙𝐼 + 𝑷𝐷
𝑇 𝒙𝐷,
(37.12)
(37.13)
and the space of admissible virtual displacements is that of any 𝛿𝒙𝐼. The criterion for a 
valid partitioning is that the 𝑚 × 𝑚 matrix given by 
𝑇 ,
𝑪𝐷 = 𝑪𝑷𝐷
(37.14)
is  non-singular,  which  is  always  possible  unless  there  are  conflicting  or  redundant 
constraints.    The  Linear  Constraint  PACKage  (LCPACK)  in  LS-DYNA  performs  this 
partitioning  and  invalid  constraints  will  result  in  error  termination.    Introducing  the 
𝑚 × (𝑛 − 𝑚) matrix 
we can combine the variations of (37.10) and (37.13) and use (37.14) and (37.15) to obtain 
𝑪𝐼 = 𝑪𝑷𝐼
(37.15)
𝛿𝒙 = 𝑷𝑇𝛿𝒙𝐼,
(37.16)
where
LS-DYNA Theory Manual 
Implicit 
𝑇𝑪𝐷
is  a  projection-like  matrix  from  the  global  variable  space  to  the  independent  solution 
space.    Using  this  expression  for  𝛿𝒙  in  the  principle  of  virtual  work  (37.7),  the 
arbitrariness of 𝛿𝒙𝐼 results in  
𝑷 = 𝑷𝐼 − 𝑪𝐼
−𝑇𝑷𝐷
(37.17)
with 
𝑸 = 𝟎,
𝑸 = 𝑷(𝑹 + 𝑪𝜆
𝑇𝝀).
(37.18)
(37.19)
This can be interpreted as to solve for zero force in the direction of deformation that is 
not  constrained,  in  other  directions  the  constraints  induce  reaction  forces  that  are 
typically  monitored  in  the  LS-DYNA  ascii  and  binout  databases  associated  with  the 
constraint  type.    The  reaction  forces  corresponding  to  those  constraints  of  the  second 
kind is contained in 𝝀. 
37.2.3  Reaction forces due to constraints 
Alternatively, we may form the lagrangian ℒ for the entire system as 
ℒ(𝒙, 𝝀, 𝑡) = ℇ(𝒙, 𝑡) + 𝝀𝑇𝑯(𝒙, 𝑡)
(37.20)
where ℇ is an assumed potential for the residual force 𝑹. It is important to stress that the 
potential  may  not  exist  in  general,  this  requires  that  the  system  is  conservative  in  the 
sense of e.g. hyperelasticity.  But it serves the purpose here for deriving the Lagrangian 
multiplier 𝝀 and subsequently the reaction forces due to the constraints 𝑯. The Karush-
Kuhn-Tucker conditions for equilibrium is now (omitting arguments) 
𝑹 + 𝑪𝑇𝝀 = 𝟎
= 𝟎
(37.21)
where  𝝀  is  a  vector  of  length  𝑚  to  be  interpreted  as  the  resisting  force  needed  to 
maintain  the  constraints.  Continuing,  we  split  𝑹  and  𝑪  into  their  respective 
independent and dependent parts, leading to a rewrite of the first of (37.21) 
𝑹𝐼 + 𝑪𝐼
𝑹𝐷 + 𝑪𝐷
𝑇𝝀 = 𝟎
𝑇 𝝀 = 𝟎
(37.22)
from which the Lagrangian multipliers can be solved from the second of (37.22) as 
𝝀 = −𝑪𝐷
−𝑇𝑹𝐷.
(37.23)
This  is  the  (generalized)  force  needed  to  enforce  the  second  of  (37.21).  To  obtain  the 
corresponding nodal (reaction) force vector associated with a single constraint 𝑗 ∈ [1, 𝑚] 
we form
Implicit 
LS-DYNA Theory Manual 
𝒓𝑗 = 𝜆𝑗𝒄𝑗
(37.24)
where  𝒄𝑗  is  the  𝑗:th  row  in  the  constraint  matrix  𝑪,  and  𝜆𝑗  is  the  corresponding 
component  of  𝝀.  These  are  the  equations  that  form  the  basis  for  the  detailed  database 
outputs, such as bndout in the case of prescribed motion. 
37.3  Implicit Statics 
37.3.1  Linearization 
For the implicit static solution 𝑴 = 𝟎 in (37.1) and the residual and constraint vector at a 
given time 𝑡 becomes an implicit function of 𝒙 only.  We seek the vector 𝒙 and multiplier 
𝝀 such that (37.8) and (37.10) holds together with 
𝑸(𝒙, 𝝀) = 𝟎.
(37.25)
Assume an approximation 𝒙𝑘 to 𝒙 and 𝝀𝑘 to 𝝀 for 𝑘 = 1, 2, 3...etc.  In the neighborhood of 
𝒙𝑘 and 𝝀𝑘 we use a linear approximation to (37.10) and (37.25) given by 
𝑘 + 𝑷𝑪𝜆
𝑇𝛥𝝀𝑘 = 𝑭(𝒙𝑘, 𝝀𝑘),
𝑲(𝒙𝑘)𝛥𝒙𝐼
(37.26)
and iterate for the solution 
𝑘+1 = 𝒙𝐼
𝒙𝐼
𝑘,
𝑘 + 𝑠𝛥𝒙𝐼
𝝀𝑘+1 = 𝝀𝑘 + 𝑠𝛥𝝀𝑘
(37.27)
Here  𝑠  is  a  convenient  step  size  to  be  discussed  below,  as  will  be  the  update  of  the 
𝑘+1. The linear system (37.26) is derived using the assumption that 𝑷 is 
dependent part 𝒙𝐷
independent  of  𝒙,  which  is  generally  not  true.    Many  constraints  in  LS-DYNA  are 
nonlinear  and  a  strict  linearization  would  have  to  take  the  second  variation  of 
constraints into account.  But this would be inherently complex, thus linearizing (37.25) 
using (37.19) just becomes 
𝑸(𝒙𝑘+1, 𝝀𝑘+1) ≈ 𝑸(𝒙𝑘, 𝝀𝑘) + 𝑷
𝜕𝑹
𝜕𝒙
To  be  able  to  solve  for  ∆𝒙𝑘  and  Δ𝝀𝑘 this  needs  first  to  be  combined  with  a  linearized 
equation of the constraint (37.10) 
(𝒙𝑘)∆𝒙𝑘 + 𝑷𝑪𝜆
𝑇𝛥𝝀𝑘 = 𝟎. 
(37.28)
𝑯(𝒙𝑘+1) ≈ 𝑯(𝒙𝑘) + 𝑪(𝒙𝑘)∆𝒙𝑘 = 𝟎,
(37.29)
and an incremental correspondent to (37.13) 
𝑘 + 𝑷𝐷
These  last  two  equations  together  with  (37.14)  and  (37.15)  can  be  used  to  yield  an 
expression for the dependent part of the displacement increment 
∆𝒙𝑘 = 𝑷𝐼
𝑘 .
𝑇 ∆𝒙𝐷
𝑇∆𝒙𝐼
(37.30)
−1(𝒙𝑘)[𝑯(𝒙𝑘) + 𝑪𝐼(𝒙𝑘)∆𝒙𝐼
Using (19.22) in (37.30) in (37.28) results in expressions of the vector 𝑭 and jacobian 𝑲 in 
(37.26) as 
𝑘 = −𝑪𝐷
(37.31)
∆𝒙𝐷
𝑘].
LS-DYNA Theory Manual 
𝑭(𝒙𝑘, 𝝀𝑘) = −𝑸(𝒙𝑘, 𝝀𝑘) + 𝑷
𝜕𝑹
𝜕𝒙
and 
(𝒙𝑘)𝑷𝐷
𝑇 𝑪𝐷
−1(𝒙𝑘)𝑯(𝒙𝑘)
𝑲(𝒙𝑘) = 𝑷
𝜕𝑹
𝜕𝒙
(𝒙𝑘)𝑷𝑇.
Implicit 
(37.32)
(37.33)
The  dependent  part  of  the  solution  vector  is  in  general  analogous  to  (37.27)  of  the 
indendent part 
𝑘 + 𝑠∆𝒙𝐷
except for those constraint equations where there is an explicit expression 𝒙𝐷 = 𝒙𝐷(𝒙𝐼), 
then of course 
𝑘+1 = 𝒙𝐷
𝒙𝐷
(37.34)
𝑘+1 = 𝒙𝐷(𝒙𝐼
𝒙𝐷
𝑘+1).
(37.35)
The  constraint  vector  corresponding  to  those  of  the  second  kind  needs  also  to  be 
linearized,  
𝑯𝜆(𝒙𝑘+1) ≈ 𝑯𝜆(𝒙𝑘) + 𝑪𝜆(𝒙𝑘)∆𝒙𝑘 = 𝟎,
(37.36)
and repeating the same procedure as above, we are lead to 
𝑪𝜆(𝒙𝑘)𝑷𝑇∆𝒙𝐼
𝑘 = 𝑮(𝒙𝑘)
with 
𝑮(𝒙) = −𝑯𝜆(𝒙) + 𝑪𝜆(𝒙)𝑷𝐷
𝑇 𝑪𝐷
−1(𝒙)𝑯(𝒙),
(37.37)
(37.38)
which  completes  the  linearization.    In  sum,  the  Newton  step  thus  means  solving  the 
combined  system  (37.26)  and  (37.37)  for  ∆𝒙𝑘  and  ∆𝝀𝑘  and  update  the  solution  using 
(37.27).  For  simplicity,  we  will  hereforth  assume  𝑚𝜆 = 0,  i.e.,  all  constraints  are  of  the 
first kind, to simplify the exposition. 
from 
The jacobian matrix 𝑲 is the assembly of the tangent moduli of materials, external loads, 
contacts, etc., and is in practice only an approximation due to the complexity of taking 
all dependencies into account.  In particular it does not include the geometric stiffness 
contribution 
on  CON-
TROL_IMPLICIT_GENERAL.  A  speculative  reason  is  that  this  has  a  smoothing  effect 
and  eliminates  negative  eigenvalues  due  to  compressive  stresses.    If  the  deformation 
mode is known to be mainly in tension or if the material is hyper-elastic, including the 
geometric  stiffness  could  improve  convergence  however.    Often  the  stiffness  matrix  is 
assumed  symmetric  and  positive  definite,  but  is  not  limited  to  those  characteristics.  
internal 
default, 
forces 
IGS 
see 
by
Implicit 
LS-DYNA Theory Manual 
Note also that (37.32) indicates that both 𝑸 and 𝑯 must vanish to render a zero 𝑭, thus a 
zero displacement increment ∆𝒙 in the iterative scheme. 
Figure 3737-1 Linear axial buckling of an aluminium beverage can. 
37.3.2  Linear theory 
For a linear solution, (37.26) is solved once to obtain the linear displacement vector 𝒖 =
∆𝒙, and often the following assumptions apply.  The configuration 𝒙 to which the linear 
approximation apply is stress free and all constraints are fulfilled, so the right hand side 
𝑭  in  (37.32)  is  essentially  the  external  applied  load  𝑭𝑒,  𝑭 = 𝑷𝑭𝑒,  which  is  constant.  
Furthermore, 𝑷 is constant due to trivial constraints and the stiffness matrix 𝑲 in (37.33) 
thus evaluates from the linearization of internal forces 
𝑲 = 𝑷 ∫ 𝑩𝑇𝑬𝑩𝑑𝑉
𝑷𝑇, 
(37.39)
𝜕𝜺  to  denote  the  constitutive  matrix.    So  in  more  conventional 
where  we  used  𝑬 = 𝜕𝝈
terms, the linear equation is written 
𝑲𝒖 = 𝑭.
(37.40)
Once solved, the stress 
𝝈 = 𝑬𝑩𝒖
(37.41)
can be evaluated from the constitutive law for the resulting deformation.  The stiffness 
matrix 𝑲 in (37.40) is symmetric and positive definite if 𝑬 is and 𝑷 eliminates all rigid 
body  modes,  whence  the  solution  𝒖  is  unique.    Furthermore,  linearity  implies  that 
substituting  the  right  hand  side  for  𝑭𝜆 = 𝜆𝑭,  the  solution  changes  to  𝒖𝜆 = 𝜆𝒖  and  the 
resulting stress changes to 
linear 
A 
TROL_IMPLICIT_SOLUTION. 
solution 
is 
𝝈𝜆 = 𝜆𝝈. 
by 
obtained 
putting  NSOLVR = 1 
(37.42)
on  CON-
LS-DYNA Theory Manual 
Implicit 
Now go back to the nonlinear static equation and scale a constant external load 𝑭𝑒 with 𝜆  
(37.43)
and assume an updated configuration 𝒙𝜆 with resulting stress 𝝈𝜆 to be the solution.  To 
see how the solution changes with 𝜆 we can perturb (37.43) to obtain 
𝑷[𝑭𝑖 − 𝜆𝑭𝑒] = 𝟎 
𝑷 [
𝜕𝑭𝑖
𝜕𝒙
𝑷𝑇𝛿𝒙𝜆 − 𝛿𝜆𝑭𝑒] = 𝟎 
(37.44)
where we applied (37.16). This is conveniently rewritten as 
(37.45)
where the presence of stress will change the evaluation of the stiffness matrix from that 
in (37.39) to 
𝑲𝜆𝛿𝒙𝜆 = 𝛿𝜆𝑭, 
𝑲𝜆 = 𝑲 + 𝑷 ∫ 𝓑 𝑇𝝈𝜆𝓑𝑑𝑉
𝑷𝑇. 
(37.46)
Here the second term is the geometric contribution to the tangent stiffness matrix where 
𝓑  is  a  matrix  consisting  of  shape  function  derivatives  for  the  finite  element.    We  are 
interested  in  the  question  of  uniqueness  of  𝛿𝒙𝜆  as  the  solution  to  (37.45),  and  this 
uniqueness is lost when 
(37.47)
If one assumes that deformations are small enough to keep 𝑉, 𝑩, 𝑬 and 𝓑 independent 
of  𝜆,  and  that  (37.42)  holds  with  (37.41)  and  (37.40),  then  (37.47)  can  be  stated  as  the 
following eigenvalue problem 
det(𝑲𝜆) = 0. 
with the geometric (nonlinear) stiffness matrix given by 
𝑲𝛿𝒖 = −𝜆𝑲𝜎𝛿𝒖 
𝑲𝜎 = 𝑷 ∫ 𝓑 𝑇𝝈𝓑𝑑𝑉
𝑷𝑇 
(37.48)
(37.49)
and  𝑲  is  the  material  (linear)  stiffness  matrix  again  given  by  (37.39).  This  is  the  theory 
behind linear buckling, see CONTROL_IMPLICIT_BUCKLE, with 𝜆 being the buckling 
load parameter and 𝛿𝒖 the associated buckling mode.  Usually solutions with 𝜆 > 0 are 
of interest, and from (37.48) and (37.49) it then follows that the principal stresses cannot 
be  positive  throughout  the  domain  of  integration.    In  other  words,  the  model  must 
somehow be in a compressed state.  The full procedure is  
1.Assemble 𝑲 by (37.39). 
2.Solve (37.40) for a constant reference load 𝑭. 
3.Evaluate resulting stress 𝝈 by (37.41). 
4.Assemble 𝑲𝜎 by (37.49). 
5.Solve (37.48) for 𝜆 and 𝛿𝒖. 
An example of linear buckling is shown in Figure 3737-1, simulating the stepping on an 
aluminium beverage can.
Implicit 
LS-DYNA Theory Manual 
𝐹 
𝐹0
𝐹0 
𝐹1 
𝐹2 
𝑥2 
𝑥1 
𝑥0
𝐹1 
𝐹2
𝑥2 
𝑥1 
𝑥0 
Figure  3737-2  Full  Newton  (left)  compared  to  quasi-Newton  secant  updates 
(right),  the  linear  approximation  to  obtain  𝑥2  is  for  full  Newton  the  exact 
tangent  in  (𝑥1, 𝐹1)  while  it  is  the  linear  extension  between  the  points  (𝑥0, 𝐹0)
37.3.3  Quasi-Newton iterations 
Now back to the nonlinear theory.  To obtain the solution at load increment 𝑗 + 1 given 
the solution at load increment 𝑗, linearized equations of the form 
𝑲𝑘𝛥𝒙𝑘 = 𝑭𝑘,
(37.50)
are assembled and solved where 𝑘 is the iteration number and 
𝑲𝑘 = Tangent stiffness matrix 
Δ𝒙𝑘 = Desired increment in displacements 
𝑭𝑘 = Residual load vector. 
This  should  be  seen  a  generalization  of  (37.26)  in  the  sense  that  the  tangent  stiffness 
matrix 𝑲 need not be calculated as (37.33) but can be based on other approximations to 
be presented.  We do however assume, without loss of generality, that (37.50) is in the 
independent  system  of  variables  so  the  residual  vector  𝑭  is  given  by  (37.32).  We  here 
just  substitute  the  sub-index  𝐼  in  the  incremental  displacement  ∆𝒙  for  the  iteration 
counter 𝑘 to simplify the notation in the following.  The coordinate vector is updated 
𝒙𝑘+1 = 𝒙𝑘 + sΔ𝒙𝑘,
(37.51)
where 𝑠 is a parameter between 0 and 1 found from a line search. 
If the tangent stiffness matrix is calculated as (37.33) for each 𝑘 then this is termed a full 
Newton method, but it may be beneficial to use so called quasi-Newton updates of 𝑲−1 to 
avoid  the  cost  of  solving  a  linear  system  of  equations  in  each  iteration.  Four  such 
methods for updating the stiffness matrix are available 
•  Broyden’s first method
LS-DYNA Theory Manual 
Implicit 
•  Davidon 
•  DFP 
•  BFGS 
and  these  involve  rank  1  or  rank 2  stiffness  updates.    Quasi-Newton  methods  are  less 
expensive than the full Newton method but often still result in robust program.  In one 
dimension,  quasi-Newton  corresponds  to  secant  iterations  and  this  method  compared 
to full Newton is illustrated in Figure 3737-2.  Henceforth we assume that 𝑲0 represents 
the  last  assembled  matrix  according  to  (37.33)  and  then  𝑲𝑘,  𝑘 = 1,2,3, …  are  quasi-
Newton updates to be given in the following. 
The secant matrices 𝑲𝑘 are found via the quasi-Newton equations 
where 
𝑲𝑘Δ𝒙𝑘−1 = Δ𝑭𝑘,
Δ𝑭𝑘 = 𝑭𝑘−1 − 𝑭𝑘.
(37.52)
(37.53)
Two  classes  of  matrix  updates  that  satisfy  the  quasi-Newton  equations  are  of  interest; 
rank 1 updates 
and rank 2 updates 
𝑲𝑘 = 𝑲𝑘−1 + 𝛼𝒛𝒚𝑇,
𝑲𝑘 = 𝑲𝑘−1 + 𝛼𝒛𝒚𝑇 + 𝛽𝒗𝒖𝑇.
Substituting (37.54) into (37.52) gives 
𝑲𝑘−1𝛥𝒙𝑘−1 + 𝛼𝒛𝒚𝑇𝛥𝒙𝑘−1 = 𝛥𝑭𝑘.
(37.54)
(37.55)
(37.56)
By  choosing  𝛼 = 1
𝒚𝑇𝛥𝒙𝑘−1
arbitrary vector but is restricted such that 
    and  𝒛 = −𝑭𝑘,  equation  (37.52)  is  satisfied.    Note  that  𝒚  is  an 
The tangent stiffness update is 
𝒚𝑇𝛥𝒙𝑘−1 ≠ 0.
𝑲𝑘 = 𝑲𝑘−1 −
𝑭𝑘𝒚𝑇
𝒚𝑇𝛥𝒙𝑘−1
,
(37.57)
(37.58)
resulting generally in non-symmetric secant matrices.  The inverse forms are found by 
the Sherman-Morrison formula 
(𝑨 + 𝒂𝒃𝑇)
−1
= 𝑨−1 −
𝑨−1𝒂 𝒃𝑇𝑨−1
1 + 𝒃𝑇𝑨−1𝒂
.
(37.59)
where  𝑨  is  a  nonsingular  matrix  and  𝒂  and  𝒃  are  arbitrary  vectors  such  that  1 +
𝒃𝑇𝑨−1𝒂 ≠ 0.  The inverse form for (37.58) can be found by letting 
𝑨 = 𝑲𝑘−1, 𝒂 =
−𝑭𝑘
𝒚𝑇𝛥𝒙𝑘−1
, 𝒃 = 𝒚,
(37.60)
Implicit 
LS-DYNA Theory Manual 
in the Sherman-Morrison formula.  Therefore, 
𝑲𝑘
−1 =
[𝑲𝑘−1
⎢⎡𝑰 +
⎣
−1 𝑭𝑘]𝒚𝑇
𝒚𝑇𝛥𝑭𝑘
Broyden´s  method  use 𝒚 = ∆𝒙𝑘−1  resulting  in  non-symmetric  stiffness  updates,  and  an 
algorithm for this exploits that 
𝒅𝑘∆𝒙𝑘−1
 𝛾𝑘
𝒅𝑘−1∆𝒙𝑘−2
𝛾𝑘−1
𝒅1∆𝒙0
𝛾1
⎥⎤ 𝑲𝑘−1
−1 .
⎦
−1 = [𝑰 +
] … [𝑰 +
] [𝑰 +
] 𝑲0
−1 
𝑲𝑘
(37.61)
(37.62)
where 
(37.63)
To illustrate the efficiency of a quasi-Newton method we outline the steps to obtain ∆𝒙𝑘. 
1.Assume ∆𝒙0, 𝑭𝑘 and 𝑭𝑘−1 (recalling (37.53)) are known, as well as ∆𝒙𝑖, 𝒅𝑖 and 𝛾𝑖 for 
𝛾𝑘 = ∆𝒙𝑘−1
𝒅𝑘 = 𝑲𝑘−1
𝑇 ∆𝑭𝑘.
−1 𝑭𝑘,
𝑖 = 1, … , 𝑘 − 1. 
−1𝑭𝑘. 
2.Solve 𝒆0 = 𝑲0
3.Recursively compute 𝒆𝑖 = 𝒆𝑖−1 +
𝑇 ∆𝑭𝑘. 
4.Set 𝒅𝑘 = 𝒆𝑘−1 and 𝛾𝑘 = ∆𝒙𝑘−1
𝑇 𝒅𝑘
∆𝒙𝑘−1
] 𝒅𝑘. 
5.Compute ∆𝒙𝑘 = [1 +
𝛾𝒌
𝑇 𝒆𝑖−1
∆𝒙𝑖−1
𝛾𝒊
𝒅𝑖 for 𝑖 = 1, … , 𝑘 − 1. 
Noteworthy here is that an iteration consists of a forward and backward substitution of 
an  already  factorized  matrix  (step  2)  plus  a  sequence  of  vector  operations  (steps  3-5), 
which  altogether  presumably  is  much  less  expensive  than  solving  an  entire  system  of 
linear equations.  The algorithm requires an in-core storage consisting of 2𝑘 vectors and 
𝑘 scalars to complete iteration 𝑘. 
Again, recalling the quasi-Newton equation (37.52), and substituting (37.55) gives 
𝑲𝑘−1𝛥𝒙𝑘−1 + 𝛼𝒛𝒚𝑇𝛥𝒙𝑘−1 + 𝛽𝒗𝒖𝑇𝛥𝒙𝑘−1 = 𝛥𝑭𝑘,
,  𝒛 = −𝑭𝑘−1,  𝛽  = 1
  and  𝒗 = 𝛥𝑭𝑘.  Here    𝒚  and  𝒖  are  arbitrary 
(37.64)
and  set  𝛼  = 1
vectors that are non-orthogonal to 𝛥𝒙𝑘−1, i.e., 
𝒚𝑇𝛥𝒙𝑘−1
𝒖𝑇𝛥𝒙𝑘−1
and 
In the BFGS method 
𝒚𝑇𝛥𝒙𝑘−1 ≠ 0,
𝒖𝑇𝛥𝒙𝑘−1 ≠ 0.
which leads to the following update formula 
𝒚 = 𝑭𝑘−1
𝒖 = 𝛥𝑭𝑘,
𝑲𝑘 = 𝑲𝑘−1 +
𝛥𝑭𝑘𝛥𝑭𝑘
𝛥𝒙𝑘−1
𝑇 𝛥𝑭𝑘
−
𝑭𝑘−1𝑭𝑘−1
𝑇 𝑭𝑘−1
𝛥𝒙𝑘−1
,
(37.65)
(37.66)
(37.67)
(37.68)
that  preserves  symmetry  of  the  secant  matrix.    A  double  application  of  the  Sherman-
Morrison formula then leads to the inverse form.
LS-DYNA Theory Manual 
Implicit 
Special product forms have been derived for the DFP and BFGS updates and exploited 
by Matthies and Strang [1979], 
𝑲𝑘
 −1 = [𝑰 + 𝒒𝑘𝒑𝑘
𝑇] 𝑲𝑘−1
−1 [𝑰 + 𝒑𝑘𝒒𝑘
𝑇].
(37.69)
The primary advantage of the product form is that the determinant of 𝑲𝑘 and therefore, 
the  change  in  condition  number  can  be  easily  computed  to  control  updates.    The 
updates vectors are defined as 
𝒑𝑘 = −𝛥𝑭𝑘 − 𝑭𝑘−1√
𝛥𝒙𝑘−1
𝛥𝒙𝑘−1
𝑇 𝛥𝑭𝑘
𝑇 𝑭𝑘−1
,
𝛥𝒙𝑘−1
𝑇 𝛥𝑭𝑘
Noting that the determinant of 𝑲𝑘 is given by 
𝛥𝒙𝑘−1
𝒒𝑘 =
.
det(𝑲𝑘) = det(𝑲𝑘−1)[1 + 𝒒𝑘
𝑇𝒑𝑘]
,
it can be shown that the change in condition number, 𝑐, is 
𝑐 =
[√𝒑𝑘
𝑇𝒑𝑘 𝒒𝑘
𝑇𝒒𝑘 + √𝒑𝑘
𝑇𝒑𝑘 𝒒𝑘
𝑇𝒒𝑘 + 4 (1 + 𝒑𝑘
𝑇𝒒𝑘 )]
𝑇𝒒𝑘)]
[4 (1 + 𝒑𝑘
(37.70)
(37.71)
(37.72)
(37.73)
. 
Following the approach of Matthies and Strang [1979] this condition number is used to 
decide  whether  or  not  to  do  a  given  update.    The  quasi-Newton  condition  (37.52)  is 
easily  verified  using  (37.69)  for  a  real  non-singular  tangent  matrix  𝑲𝑘−1  and  it  follows 
that  BFGS  preserves  not  only  symmetry  but  also  positive  definiteness.    Interestingly 
enough  the  converse  is  not  true;  if  𝑲𝑘−1  is  indefinite  then  𝑲𝑘  may  still  be  positive 
definite. 
An algorithm would utilize that 
𝑲𝑘
𝑇], 
𝑇]𝑲0
−1[𝑰 + 𝒑1𝒒1
𝑇] … [𝑰 + 𝒒1𝒑1
−1 = [𝑰 + 𝒒𝑘𝒑𝑘
𝑇] … [𝑰 + 𝒑𝑘𝒒𝑘
(37.74)
−1𝑭𝑘  requires  a  sequence  of  vector  operations,  followed 
so  the  computation  of  ∆𝒙𝑘 = 𝑲𝑘
by a forward and backward substitution of a factorized matrix, followed by yet another 
sequence  of  vector  operations.    The  BFGS  algorithm  requires  an  in-core  storage  of  the 
vectors  𝒑𝑖  and  𝒒𝑖,  𝑖 = 1, … , 𝑘 − 1,  and  ∆𝒙𝑘−1  and  𝑭𝑘−1  to  complete  iteration  𝑘.  It  is  the 
default and most robust quasi-Newton algorithm for the nonlinear implicit solver and 
there is no reason to switch.  The only practical issue is how to control when to reform 
the tangent stiffness matrix, which typically depends on the degree of nonlinearity for 
the  problem  at  hand.    In  fact,  if  LCPACK = 2  on  CONTROL_IMPLICIT_SOLVER,  i.e., 
working  with  independent  variables  only,  BFGS  is  mandatory  and  comes  in  two 
flavors, NSOLVR = 2 or NSOLVR = 12 on CONTROL_IMPLICIT_SOLUTION. 
There is also the option LCPACK = 3, for which LS-DYNA uses a non-symmetric matrix 
assembly when solving the linear system of equations.  This adds to the computational
Implicit 
LS-DYNA Theory Manual 
cost for each iteration but my improve convergence because of better tangents of certain 
features.    The  non-symmetric  solver  is  illustrated  in  Figure  3737-3  for  simulating  a 
clamped  cantilever  beam  subject  to  a  follower  load.    In  general  the  stiffness  matrix  is 
symmetric  when  the  force  is  derived  from  an  energy  potential,  or  in  other  words  is 
conservative.  This  is  for  instance  the  case  for  a  hyperelastic  material  response  or  a 
physically  admissible  pressure  load,  see  Schweizerhof  and  Ramm  [1984]  for  a 
discussion.    Non-symmetry  arise  e.g.  from  non-conservative  forces,  such  as  frictional 
contact,  or  physically  inadmissible  design  dependent  loads.    The  example  in  Figure 
3737-3  serves  as  one  of  the  latter  since  the  load  is  not  coming  from  a  physical  source, 
such  as  a  water  pressure,  and  it  should  be  seen  as  an  academic  example  to  prove  a 
point. 
Follower load 𝐹 
𝐹 = 1/16 
𝐹 = 1/4
𝐹 = 1/2
𝐹 = 1 
Figure  3737-3  Nonlinear  implicit  solution  of  an  elastic  cantilever  beam  with  a 
follower force, von Mises stress is fringed.. 
37.3.4  Tangent stiffness reformations 
In  the  previous  section  we  have  used  𝑲0  in  (37.62)  and  (37.74)  to  represent  the  last 
assembled  tangent  stiffness  matrix  according  to  (37.33).  While  the  quasi-Newton 
updates 𝑲𝑘, 𝑘 = 1,2, … are justified in the context of moderate nonlinearities and/or for 
a few iterations, it will eventually break down convergence for more complex problems.  
Whence there are criteria for reforming the tangent stiffness matrix and start over with 
the quasi-Newton (BFGS) updates. 
The  first  criterion  is  simply  a  user  defined  upper  limit  of  𝑘,  governed  by  ILIMIT  on 
CONTROL_IMPLICIT_SOLUTION.  Using  ILIMIT = 1  means  that  no  quasi-Newton 
updates are performed and should be used for highly nonlinear problems, larger values
LS-DYNA Theory Manual 
Implicit 
of ILIMIT can be used if the nonlinearities are considered less severe.  ILIMIT = 11 is the 
default and is a reasonable value to use for starters. 
A second criterion is that of increased residual norm, i.e., if any of the quantities 
𝑇𝑘 = ‖𝑱𝑡𝑭𝑘‖1 
(37.75)
or 
𝑅𝑘 = ‖𝑱𝑟𝑭𝑘‖1 
(37.76)
for some 𝑘 is their respective largest attained since start iterating, the stiffness matrix is 
reformed.  Here 𝑱𝑡 and 𝑱𝑟 are diagonal matrices with ones or zeros on the diagonal that 
extract the translational and rotational degrees of freedom, respectively, and one speaks 
of translational or rotational divergence.  The notation ‖𝑭‖1 indicates the 𝐿1-norm of 𝑭, 
meaning the sum of the absolute value of its components. 
A third criterion is called energy explosion, if 
log(1 + ∣∆𝒙𝑘−1
𝑇 𝑱𝑡𝑭𝑘−1∣) + log(1 + ∣∆𝒙𝑘−1
𝑇 𝑱𝑡𝑭𝑘∣) > 36 
(37.77)
or 
log(1 + ∣∆𝒙𝑘−1
(37.78)
the stiffness matrix is reformed.  One can speak also here of translational and rotational 
energy  explosion  and  this  simply  indicates  that  something  really  bad  has  happened 
with the last search direction. 
𝑇 𝑱𝑟𝑭𝑘−1∣) + log(1 + ∣∆𝒙𝑘−1
𝑇 𝑱𝑟𝑭𝑘∣) > 36 
Finally, a necessary criterion for continuing with BFGS updates is deemed 
∆𝒙𝑘
(37.79)
since  this  would  otherwise  indicate  a  search  direction  corresponding  to  a  zero  or 
negative  eigenvalue  in  the  tangent  matrix.    If  this  criterion  is  violated  the  tangent 
stiffness  matrix  is  reformed  with  a  warning  message  issued  that  negative  energy  is 
detected  during  quasi-Newton  updates.    This  can  only  happen  if  there  are  negative 
eigenvalues in the tangent stiffness matrix in the first place. 
𝑇𝑭𝑘 > 0
37.3.5  Line search 
Line  search  is  critical  for  decent  convergence  characteristics,  and  there  are  several 
criteria to choose from, see LSMTD and LSTOL on CONTROL_IMPLICIT_SOLUTION. 
One  of  the  criteria  available  is  that  the  norm  of  residual  𝑭  must  somehow  decrease, 
LSMTD = 2,  but  this  will  inevitably  lead  to  ridiculously  small  steps  and  is  not 
recommended  or  presented  further  here.    A  more  useful  criterion  is  instead  that  an 
iterate 𝑘 + 1 is accepted if 
𝑇𝑭𝑘 
𝑇𝑭𝑘+1∣ ≤ 𝜀𝑠∆𝒙𝑘
∣∆𝒙𝑘
(37.80)
where  𝜀𝑠  is  the  line  search  convergence  tolerance  LSTOL.  See  Figure  3737-4  for  an 
illustration.  This criterion is derived from a hypothetical assumption of the existence of 
an  energy  potential  𝑊(𝒙𝑘 + 𝑠∆𝒙𝑘)  for  the  residual  force  𝑭  and  that  the  potential  is 
minimized along the search direction 
𝜕𝑊
𝜕𝒙
= 𝑭 𝑇∆𝒙𝑘 = 0. 
𝜕𝑊
𝜕𝑠
(37.81)
𝜕𝒙
𝜕𝑠
=
Implicit 
LS-DYNA Theory Manual 
𝑇∆𝒙𝑘 
𝑭𝑘
𝑭 𝑇∆𝒙𝑘 
(1.60) not solvable 
Acceptable interval 
according to (37.80) 
𝜀𝑠𝑭𝑘
𝑇∆𝒙𝑘 
𝑠 
𝑠 = 1
Negative starting values 
indicate negative 
eigenvalues in tangent 
Figure  3737-4  Illustration  of  line  search  based  on  energy,  may  be 
complemented  with  norm  of  𝑭.  Dashed  line  indicates  a  line  search  that 
So in a sense, (37.80) is the solution of (37.81) to within a certain tolerance and a Ridder 
algorithm is used to narrowing in on a candidate.  It is not unusual however that (37.80) 
is not well-posed, an indefinite stiffness matrix may result in a negative right hand side 
or the search direction may be bad enough to not render a solution, see Figure 3737-4. In 
those special cases some conservative approach is taken to provide a reasonable iterate 
𝑘 + 1. This summarizes in brief LSMTD = 4. 
A  closer  examination  (and  numerical  experiments)  reveals  that  𝑭𝑘+1  is  not  necessarily 
bounded by (37.80). Therefore this criterion can be complemented with  
∥𝑭𝑘+1∥1 ≤ [1 + 𝜀𝑠]‖𝑭𝑘‖1.
(37.82)
where again ‖𝑭‖1 means the 𝐿1-norm of 𝑭. This option is invoked with LSMTD = 5 and 
means  that  both  (37.80)  and  (37.82)  are  to  be  satisfied  for  accepting  an  iterate  𝑘 + 1. 
While  this  is  a  more  robust  approach,  it  also  requires  more  residual  force  evaluations 
and  is  not  recommended  as  default.    It  has  proved  to  work  well  for  implicit  rubber 
simulations and complicated contact problems. 
37.3.6  Convergence check 
Convergence  criteria  are  based  on  displacement,  energy  and  residual  force  quantities.  
The  exact  definitions  of  norms  and  scalar  products  used  depend  to  a  great  extent  on 
parameter  settings  on  CONTROL_IMPLICIT_SOLUTION, 
in  particular  on  the 
parameter  NLNORM.  Historically  it  has  been  assumed  that  rotational  degrees  of 
freedom are not appropriate for checking convergence and therefore only translational 
degrees of freedom have been considered.  With advancements in the development of 
the  implicit  solver,  this  is  today  considered  an  old  fashioned  way  of  thinking,  but 
backward compatibility is maintained and the user is referred to the keyword manual 
for  information  regarding  the  choices  in  this  context.    Here  the  principles  behind
LS-DYNA Theory Manual 
Implicit 
convergence checks are presented from a pragmatic standpoint assuming the following 
generic displacement and force norms and (energy) scalar products 
‖∆𝒙‖ = √∆𝒙𝑇𝑱𝑱∆𝒙,      ‖𝑭‖1 = ∑ ∣𝐽𝑖𝑖
†𝐹𝑖∣
,
〈∆𝒙, 𝑭〉 = ∆𝒙𝑇𝑱𝑱†𝑭. 
(37.83)
Note  that  the  norm  of  the  incremenetal  displacement  is  a  𝐿2-norm  (euclidian  norm) 
while the norm of the residual force is a 𝐿1-norm, this decision was made to allow for a 
more physical and less mesh dependent interpretation of this latter quantity.  Here 𝑱 is a 
diagonal matrix that appropriately scales the various degrees of freedom to account for 
units,  i.e.,  scaling  radians  with  some  characteristic  length  for  consistency.    It  also 
accounts for user input in the sense that 𝑱 may contain zeros on the diagonal to indicate 
that rotational degrees of freedom should not be accounted for. 𝑱† is the pseudo-inverse 
of  𝑱,  a  notation  introduced  since  𝑱  actually  may  be  singular  due  to  the  zeros  on  the 
diagonal.    For  some  convergence  option  check  is  performed  on  translational  and 
rotational  degrees  of  freedom  separately,  we  don’t  elaborate  on  such  details  here  but 
instead refer to the keyword manual.  In (37.83), the non-bold quantities with subscripts 
indicate components of the corresponding bold-faced vector. 
Convergence for accepting an iterate 𝑗 + 1 is assumed if the three conditions 
‖𝛥𝒙𝑘‖ < max(𝜀𝑑𝑢max, √max(𝜀𝑎, 0))
〈∆𝒙𝑘, 𝑭𝑘〉 < max(𝜀𝑒𝑒0, 10000max(𝜀𝑎, 0))
‖𝑭𝑘‖1 < max(𝜀𝑟𝑓0, 10000max(𝜀𝑎, 0)) 
(37.84
) 
(37.85
) 
(37.86)
are  satisfied  simultaneously.    Here  𝜀𝑑,  𝜀𝑒,  𝜀𝑟  and  𝜀𝑎  are  the  displacement,  energy, 
residual  and  absolute  tolerances  corresponding  to  DCTOL,  ECTOL,  RCTOL  and 
ABSTOL, respectively.  In the right hand side of (37.84), 𝑢max = ∥𝒖max∥ is the maximum 
attained displacement in any iteration 𝑘 measured from the position at the start of this 
implicit step 𝑗 if DNORM = 1 and from the start of the simulation if DNORM = 2. In the 
right  hand  side  of  (37.85),  𝑒0 = 〈∆𝒙0, 𝑭0〉  where  ∆𝒙0  and  𝑭0  are  the  first  incremental 
displacement and residual vectors for this implicit step 𝑗. Likewise 𝑓0 = ∥𝑭0∥1 in the right 
hand side of (37.86) is the norm of the first residual vector for this implicit step 𝑗. If 𝑱 has 
full rank and the tangent stiffness matrix is symmetric and positive definite then these 
conditions make intuitive sense, small changes in displacements and/or small residual 
forces indicate that an iterate is “close-enough” to the solution.  Under these conditions 
the left hand side of (37.85) define norms in both the incremental displacement ∆𝒙𝑘 and 
residual force 𝑭𝑘, and 𝑒0 > 0. 
Optionally, these convergence criteria can be combined with bounds on the maximum 
norms, here denoted 
‖∆𝒙‖∞ = max|𝑱∆𝒙|𝑖,      ‖𝑭‖∞ = max∣𝑱†𝑭∣
(37.87)
where the max is taken over all nodes and rigid bodies in the model, i.e., 𝑖 ranges over 
all  nodes  and  rigid  bodies.  If  any  of  these  options  are  activated,  then  convergence  for 
〈∆𝒙, 𝑭〉∞ = max∣∆𝒙𝑇𝑱𝑱†𝑭∣
, 
,
Implicit 
LS-DYNA Theory Manual 
accepting  an  iterate 𝑗 + 1  is  assumed  if  the  three  conditions  (37.84),  (37.85)  and  (37.86) 
are satisfied and 
‖𝛥𝒙𝑘‖∞ < 𝜀𝑑
∞𝑢max
∞
〈∆𝒙𝑘, 𝑭𝑘〉∞ < 𝜀𝑒
∞
∞𝑒0
‖𝑭𝑘‖∞ < 𝜀𝑟
∞𝑓0
∞ 
(37.88
) 
(37.89
) 
(37.90)
∞, 𝜀𝑒
∞ and 𝜀𝑟
∞ are the displacement, energy and residual tolerances 
are satisfied. Here 𝜀𝑑
corresponding  to  DMTOL,  EMTOL  and  RMTOL,  respectively,  and  if  any  of  these 
parameters are zero that means the condition is not active.  The remaining parameters 
on the right hand sides are interpreted in analogy to those appearing in the right hand 
sides  of  (37.84),  (37.85)  and  (37.86),  except  for  that  the  Euclidian  norm  is  now 
substituted for the maximum norm. 
A backdoor out is an absolute convergence test on the maximum norm on translational 
displacement.    That  is,  convergence  is  always  detected  if  the  maximum  value  of  any 
translational  degree  of  freedom  in  the  incremental  displacement  array  ∆𝒙𝑘  is  smaller 
than  𝑑√max (𝜀𝑎, 0),  where  𝑑  is  a  characteristic  size  calculated  as  the  diagonal  of  the 
smallest  box  aligned  along  the  global  coordinate  system  that  encapsulates  the  model.  
Setting  ABSTOL  to  a  negative  number  is  an  alternative,  then  all  absolute  convergence 
checks  above  become  inactive  and  instead  the  backdoor  out  is  to assume  convergence 
when  ‖𝑭𝑘‖1 < max(0, −𝜀𝑎).  This  latter  option  requires  to  some  extent  an  a  priori 
knowledge  of the  force  level  and  may  require  monitoring the  residual  norm  for  a  few 
trial iterations to pick a decent 𝜀𝑎, but it could be a sensible choice if the problem shows 
erratic behavior in displacement and energy due to severe nonlinearities.  On the other 
hand, since it is a check on the 𝐿1-norm, the value 𝜀𝑎 might be taken as some reasonable 
fraction of an external load or as an desired error on the sum of inbalanced forces. 
Another  criterion  that  must  be  met  for  convergence  is  that  simple  prescribed  motion 
constraints  on  nodes  and  rigid  bodies,  if  they  exist,  must  be  “almost”  satisfied.    The 
background  is  that  only  partial  line  searches  (𝑠 < 1)  will  not  satisfy  simple  motion 
constraints,  and  at  least  one  full  line  search step (𝑠 = 1)  must  be  accomplished  during 
the  iterations.    For  difficult  problems,  this  sometimes  never  happens  and  therefore 
convergence  is  prevented  due  to  unfulfilled  boundary  conditions  until  all  prescribed 
motion is satisfied to within 1%. 
37.3.7  Automatic time stepping 
If  convergence  is  not  attained  after  reforming  the  stiffness  matrix  a  given  amount  of 
times,  see  MAXREF  on  CONTROL_IMPLICIT_SOLUTION,  one  of  two  things  will 
happen.  By default, LS-DYNA terminates with an error message, but if automatic time 
stepping  is  turned  on,  see  IAUTO  on  CONTROL_IMPLICIT_AUTO,  then  LS-DYNA 
will  try  to  resolve  the  problem  with  a  smaller  step  size.    More  specifically,  if
LS-DYNA Theory Manual 
Implicit 
convergence  is  not  attained  with  a  time  step  ∆𝑡old,  then  LS-DYNA  backs  up  to 
beginning of step and retries with a time step 
(37.91)
where  ∆𝑡min  is  a  user  defined  minimum  step.    If  ∆𝑡old = ∆𝑡min  when  attempting  this 
then LS-DYNA will terminate with an error. 
∆𝑡new = max(∆𝑡min, 10−0.3∆𝑡old) 
With the automatic time stepper turned on, LS-DYNA will not only cut the time step for 
convergence failure but also adjust the time step when converging.  The adjustment is 
based  on  a  user  defined  iteration  window,  i.e.,  a  range  of  iteration  numbers  that  are 
deemed  acceptable  for  convergence,  and  if  the  number  of  iterations  for  convergence 
falls outside this window the next time step will be adjusted as follows.  If convergence 
is  attained  for  more  iterations  than  acceptable  then  the  time  step  for  the  next  implicit 
step is given by (37.91). If instead convergence is attained for fewer iterations then the 
next time step is given by 
∆𝑡new = min(∆𝑡max, 100.2∆𝑡old) 
(37.92)
where  ∆𝑡max  is  a  maximum  defined  step.    In  this  way  LS-DYNA  narrows  in  on  an 
optimum  time  step  for  which  the  number  of  iterations  to  converge  falls  within  the 
specified window.  
There is much more information regarding this option in the keyword manual and the 
user is referred thereto for practical issues. 
37.4  Implicit Dynamics 
37.4.1  Newmark time integration 
Nonlinear  implicit  dynamics  principally  follows  the  exact  same  solution  algorithm  as 
for nonlinear implicit statics, the only difference is that dynamic terms are included in 
the residual force.  That is, (37.1) now reads 
(37.93)
where  global  damping  is  introduced  through  the  matrix  𝑫,  so  the  residual  is  now 
essentially a function of 𝒙, 𝒙̇ and 𝒙̈. The dependence on the latter two is eliminated by 
introducing the Newmark time integration scheme 
𝑹 = 𝑴𝒙̈ + 𝑫𝒙̇ + 𝑭𝑖 − 𝑭𝑒 = 𝟎, 
𝒙̈ =
𝛥𝒙
𝛽𝛥𝑡2 −
𝒙̇𝑗
𝛽𝛥𝑡
−
(
− 𝛽) 𝒙̈𝑗,
𝒙̇ = 𝒙̇𝑗 + 𝛥𝑡(1 − 𝛾)𝒙̈ 𝑗 + 𝛾𝛥𝑡𝒙̈,
𝒙 = 𝒙𝑗 + 𝛥𝒙.
(37.94)
(37.95)
(37.96)
Here, Δ𝑡 is the time step size, 𝛽 and 𝛾 are the free parameters of integration and we have 
used ∆𝒙 to denote the total displacement from step 𝑗 to step 𝑗 + 1.  For 𝛾 = 1 ⁄ 2 and 𝛽 =
1 ⁄ 4 the method becomes the trapezoidal rule and is energy conserving.  If
Implicit 
LS-DYNA Theory Manual 
𝛾 >
,
𝛽 >
(
+ 𝛾)
,
(37.97)
(37.98)
numerical  damping  is  induced  into  the  solution  leading  to  a  loss  of  energy  and 
momentum.  By inserting (37.94) and (37.95) into (37.93) and using (37.96) to eliminate 
∆𝒙,  we  are  back  to  an  equation  in  𝒙  only  and  can  apply  the  algorithm  starting  with 
(37.25) and everything thereafter holds. 
37.4.2  Practical considerations 
Linearizing (37.93) using (37.94), (37.95) and (37.96) results in a tangent matrix 
𝜕𝑹
𝜕𝒙
=
𝛽∆𝑡2 +
𝛾𝑫
𝛽∆𝑡
+
𝜕[𝑭𝑖 − 𝑭𝑒]
𝜕𝒙
, 
(37.99)
and leads to an interesting observation.  Since 𝑴 is symmetric and positive definite the 
first term assures that the resulting tangent is positive definite as long as the time step 
∆𝑡  is  sufficiently  small,  so  including  dynamics  will  enhance  the  robustness  of  the 
numerical  procedure.    In  fact,  the  eigenvalues  of  the  resulting  tangent  can  be  made 
arbitrarily  large  by  decreasing  ∆𝑡  at  the  cost  of  requiring  more  steps  to  obtain  the 
solution. 
Not  only  robustness  but  also  the  accuracy  in  dynamic  implicit  depends  on  the  size  of 
the time step ∆𝑡, roughly speaking only frequencies up to ~∆𝑡−1 can be resolved.  The 
method  is  therefore  not  perfectly  suitable  for  contact-impact  and  restitution  problems, 
for  contact  a  crude  rule  of  thumb  is  that  the  time  a  node  or  body  is  in  contact  should 
span  at  least  a  few  time  steps  to  appropriately  resolve  the  resulting  impulse.    Having 
said this, these problems are still difficult to solve reasonably well. 
For  implicit  static  contact  problems,  a  common  usage  of  dynamics  is  to  temporarily 
suppress rigid body modes while a desired contact state is being established.  In such a 
case it is recommended to use numerical damping by for instance choosing 𝛾 = 0.6 and 
𝛽 = 0.38  to  render  a  smooth  response.    This  technique  has  proved  successful  and  it  is 
often sufficient to have dynamics initially turned on and then turned off at a time when 
all  rigid  body  modes  have  been  eliminated  by  contact.    But  it  is  also  possible  to 
arbitrarily  switch  dynamics  on  and  off  during  a  simulation,  all  this  is  explained  on 
CONTROL_IMPLICIT_DYNAMICS in the keyword manual. 
37.4.3  Linear theory 
Linearization of (37.93) with respect to a configuration 𝒙 that is in static equilibrium, i.e.,  
𝑷[𝑭𝑖 − 𝑭𝑒] = 𝟎, can be written as  
𝑴𝒖̈ + 𝑫𝒖̇ + 𝑲𝒖 = 𝑭,
(37.100)
LS-DYNA Theory Manual 
Implicit 
where we use 𝒖 = ∆𝒙 to denote the displacement measured from the reference point 𝒙. 
For the sake of clarity we also abused some notation, using 𝑴 and 𝑫 to actually mean 
𝑷𝑴𝑷𝑇 and 𝑷𝑫𝑷𝑇, respectively.  Furthermore, 𝑲 denotes the sum of the material (37.39) 
and geometric (37.49) contributions to the static tangent stiffness matrix as well as any 
contributions from the external force, e.g., contacts, 
𝑲 = 𝑷 ∫[𝑩𝑇𝑬𝑩 + 𝓑 𝑇𝝈𝓑]𝑑𝑉
𝑷𝑇 − 𝑷
𝜕𝑭𝑒
𝜕𝒙
𝑷𝑇. 
(37.101)
The right hand side 𝑭 in (37.100) should be interpreted as an external (small) load that 
only depends on time 𝑡 and serves to dynamically perturb the static equilibrium.  This 
equation can be discretized in time using the Newmark time integration scheme above 
and  then  efficiently  integrated  with  no  update  of  the  tangent  stiffness  matrix  between 
steps.  This of course assumes that the displacements 𝒖 are small enough to not affect 𝑲 
to great extent. 
Consider undamped free vibration in (37.100), i.e, 𝑫 = 𝟎 and 𝑭 = 𝟎, and transform this 
equation from time to frequency plane assuming constant 𝑴 and 𝑲. This results in an 
eigenvalue problem 
𝑲𝒖 = 𝜔2𝑴𝒖
(37.102)
that  can  be  solved  in  LS-DYNA  for  the  angular  frequency  𝜔  and  mode  shape  𝒖.  The 
stress  𝝈  in  (37.101)  affects  the  frequency  𝜔  in  the  following  way.    If  the  model  is  in  a 
tensile state, i.e., the principal stresses are positive, then the eigenvalues of  𝑲 increase 
compared  to  a  stress  free  state  and  from  (37.102)  the  frequencies  will  increase.  
Conversely,  the  frequencies  will  decrease  if  the  principal  stresses  decrease,  this  is  the 
effect  of  tuning  a  guitar  string  by  increasing  or  decreasing  its  tension.    If  linearizing 
with  respect  to  a  contact  state,  the  last  term  in  (37.101)  will  in  effect  constrain  relative 
motion  between  parts  or  nodes  in  contact.    More  specifically,  the  relative  normal 
displacement in 𝒖 will be zero, and the relative tangential motion will be governed by 
the present stick/slip condition.  If in stick mode the relative tangential displacement in 
𝒖  will  be  zero,  and 
  See  CON-
TROL_IMPLICIT_EIGENVALUE for the available options to solve (37.102). 
is  unconstrained. 
in  slip  mode 
if 
it 
An example using modal analysis in this respect is shown in Figure 37.5.
Implicit 
LS-DYNA Theory Manual 
𝑓 = 15 𝐻𝑧 
𝑓 = 40 𝐻𝑧
𝑓 = 43 𝐻𝑧
Figure 37.5.  Intermittent eigenvalue analysis of tire. Model shown in top left,
followed by lowest frequency modes for unpressurized tire (top right), inflated
tire  (bottom  left)  and  inflated  tire  and  frictional  contact  (bottom  right).
Resultant mode displacements are fringed.
LS-DYNA Theory Manual 
Implicit 
In general 𝑫 ≠ 𝟎 and 𝑫 and/or 𝑲 may be non-symmetric as discussed in Section 37.3.3, 
but we assume  𝑴 is symmetric and positive definite and still 𝑭 = 𝟎. The characteristic 
equation approach for solving (37.100) makes use of the harmonic ansatz 
which is inserted into (37.100) to yield 
𝒖(𝑡) = ∑ exp(𝜇𝑗𝑡)𝚽𝑗
∑ exp (𝜇𝑗𝑡){𝜇𝑗
2𝑴 + 𝜇𝑗𝑫 + 𝑲}𝚽𝑗
= 𝟎 
(37.103)
(37.104)
to which the quadratic eigenvalue problem is associated7 
{𝜇2𝑴 + 𝜇𝑫 + 𝑲}𝚽 = 𝟎. 
(37.105)
Because of the non-symmetry of the involved matrices, the eigenvalues to (37.105) may 
be complex but come in conjugate pairs.  That is, if 𝜇 = 𝑟 + 𝑖𝑠 is an eigenvalue then 𝜇̅̅̅̅ =
𝑟 − 𝑖𝑠 is also an eigenvalue, and if 𝚽 = 𝚼 + 𝑖𝚿 is the eigenvector associated with 𝜇 then 
𝚽̅̅̅̅̅̅ = 𝚼 − 𝑖𝚿 is the eigenvector for 𝜇̅̅̅̅. However, examining the sum of two such terms in 
(37.104) yields 
exp(𝜇𝑡){𝜇2𝑴 + 𝜇𝑫 + 𝑲}𝚽 + exp(𝜇̅̅̅̅𝑡){𝜇̅̅̅̅2𝑴 + 𝜇̅̅̅̅𝑫 + 𝑲}𝚽̅̅̅̅̅̅
= 2exp(𝑟𝑡){((𝑟2 − 𝑠2)𝑴 + 𝑟𝑫 + 𝑲)(cos(𝑠𝑡) 𝚼 − 𝑠𝑖𝑛(𝑠𝑡)𝚿)
(37.106)
− 𝑠(2𝑟𝑴 + 𝑫)(sin(𝑠𝑡) 𝚼 + cos(𝑠𝑡)𝚿)}, 
meaning  that  the  solution  in  time  domain  is  real  as  expected.    If  all  eigenvalues  are 
purely  complex,  i.e.,  𝜇𝑗 = 𝑖𝑠𝑗  and  the  real  parts  𝑟𝑗 = 0  vanish,  then  the  solution  to 
(37.100)  is  harmonic  with  angular  frequencies  𝜔𝑗 = ∣𝑠𝑗∣.  This  is  apparent  from  (37.106) 
and corresponds to the traditional solution to (37.102), with the exception of a non-zero 
damping  matrix  𝑫.  But  if  an  eigenvalue  has  a  real  part  𝑟𝑗 > 0  then  from  (37.106)  the 
solution is exponentially growing and thus unstable.  Solving (37.105) can therefore be 
used to detect instabilities in a system, eigenvalues with positive real parts correspond 
to unstable modes.  A common indicator used for this is the damp ratio defined as 
𝜗 = −2
|𝑠|
so basically a negative damp ratio indicates an unstable mode.  An application of this is 
brake  squeal,  see  Figure  37.6,  for  which  friction  instabilities  may  result  in  unwanted 
noise and erratic behavior.  Noticable is that if 𝑫 = 𝟎 and 𝜇 is an eigenvalue then – 𝜇 is 
also an eigenvalue, so then complex eigenvalues come in clusters of four, {𝜇, 𝜇̅̅̅̅, −𝜇, −𝜇̅̅̅̅}. 
Then  it  suffice  that  eigenvalues  have  nonzero  real  parts  𝑟𝑗 ≠ 0  for  a  system  to  be 
unstable, which corresponds to negative eigenvalues in (37.102). 
To solve the system (37.105), it is transformed to a first order eigenvalue problem using 
𝚽̃ = 𝜇𝚽, resulting in 
, 
(37.107)
[ 𝟎
−𝑲 −𝑫
][𝚽
𝚽̃] = 𝜇[𝑰
𝟎 𝑴
][𝚽
𝚽̃], 
(37.108)
which can be solved by well-established eigenvalue algorithms.  In the output files, LS-
DYNA reports eigenvalues with positive imaginary parts only, i.e., 𝑠𝑗 > 0, and the real 
and imaginary parts (when non-zero) of the associated eigenvector 𝚽. 
7 The eigenvalue problem (1.105) is readily obtained by Laplace transforming (1.100).
Implicit 
LS-DYNA Theory Manual 
 0.02
 0.015
 0.01
 0.005
 0
-0.005
-0.01
-0.015
-0.02
 0
 2
 4
 6
 8
 10
 12
 14
 16
Mode
Figure 37.6.  Brake squeal application.  Pressure pads are applied to a rotating
disc and a nonsymmetric eigenvalue solution reveals friction instabilities.  The
damp  ratio  𝜗  is  plotted  at  the  top  as  function  of  mode  number,  see  (37.107).
Mode #6 is the unstable mode and is depicted bottom right with displacements
fringed.
LS-DYNA Theory Manual 
Arc-length 
38    
Arc-length 
Arc-length methods are available in LS-DYNA for NSOLVR specified between 6 and 9, 
this and all other parameters in this Section are located on the *CONTROL_IMPLICIT_-
SOLUTION  keyword.  These solvers use the Riks/Crisfield methods but unfortunately 
go under the old LSDIR.EQ.1 option which makes them somewhat limited in terms of 
applicability.    For  LSDIR.EQ.2  the  arc-length  method  described  in  Ritto-Corrêa  and 
Camotim  [2008] 
implemented  for  the  combination  of  NSOLVR.EQ.12  and 
ARCMTH.EQ.3.    For  this  method  the  parameters  ARCPSI  (𝜓),  ARCALF  (𝛼)  and 
ARCTIM  apply,  out  of  which  the  last  simply  tells  at  what  time  arc-length  is  initiated 
and the first two are to be described in more detail below.  We begin by an explanatory 
overview of the arc-length method in general for which we will constantly be referring 
to Figure 38.1 below.  After that the mathematical details are revealed. 
is 
38.1  Overview 
An  implicit  static  problem  is  driven  by  a  parameter  𝑡  referred  to  as  the  time,  and 
assuming that a solution is obtained at 𝑡 = 𝑡𝑛 the objective is to determine the solution 
given the constraint 𝑡 = 𝑡𝑛+1, where 𝑡𝑛+1 is given.  We assume that the problem can be 
associated  with  representative  force  and  displacement  parameters  𝑓   and  𝑑  and  we 
distinguish  between  load-  and  displacement-driven  problems.    An  example  of  a  load-
driven problem is when 𝑓 = 𝑓 (𝑡) is an external load and 𝑑 is the resulting displacement 
of the associated nodes, and likewise a displacement-driven problem is when 𝑑 = 𝑑(𝑡) is 
a prescribed displacement and 𝑓  is the corresponding reaction force.  A solution is likely 
obtained  if  the  problem  is  stable,  i.e.,  the  force-displacement  curve  is  monotonically 
increasing,  but  this  method  is  not  designed  to  handle  limit  or  turning  points.    A  limit 
point is illustrated in figure (a) and a turning point in figure (b), the solution in the next 
step  may  not  be  the  one  desired  or  not  even  exist,  in  both  cases  we  want  to  find  the 
solution  that  continuously  follow  the  path  corresponding  to  the  force-displacement 
curve.
Arc-length 
LS-DYNA Theory Manual 
The solution for this is to set the stepping parameter 𝑡 free, i.e., replace the constraint 𝑡 =
𝑡𝑛+1  with  an  arc-length  constraint  𝑔(𝑑, 𝑓 ) = 0.    In  words,  this  basically  means  that  a 
multidimensional  sphere  (arc)  is  put  around  the  last  converged  solution  and  the  next 
solution is to be found on that given sphere, the stepping parameter 𝑡 is now a solution 
variable.    This  makes  the  problem  well-posed  but  unfortunately  there  are  multiple 
solutions  to  the  problem,  and  it  may  turn  out  that  the  wrong  solution  is  found.    In 
figures (c) and (d), the effect of the arc-length constraints is illustrated and there are two 
possible solutions, one feasible that allows us to continue in the right direction and one 
infeasible  that  takes  us  in  the  wrong  direction.    The  latter  phenomenon  is  termed 
doubling  back,  and  is  in  practice  not  easily  avoided.    Two  additional  parameters  are 
available that have shown to improve the robustness in this respect.
LS-DYNA Theory Manual 
Arc-length 
a)
b)
c)
e)
g)
d)
f)
ff
h)
Converged solution at step n
Infeasible solution at step n + 1
Feasible solution at step n + 1
Center of arc for α < 0, makes infeasible solution less probable
Figure  38.1.    Representative  force-displacement  curves  for  illustrating  arc-
length and accompanying parameters 
In figure (d), two of the infeasible solutions can in practice be avoided by including the 
stepping parameter in the arc-length constraint, thus converting a cylinder to a sphere 
in  space-time.    This  is  adjusted  by  the  paremeter  0 ≤ 𝜓 < 1,  and  the  constraint  reads 
(1 − 𝜓)𝑔(𝑑, 𝑓 ) + 𝜓(𝑡 − 𝑡𝑛)2 = 0,  the  effect  of  this  constraint  is  illustrated  in  figures  (e) 
and  (f),  and  should  be  compared  with  figures  (c)  and  (d).    Note  that  two  infeasible 
solutions are avoided when comparing figures (d) and (f), it may sometimes be worth 
using a non-zero value for 𝜓, e.g., 𝜓 = 0.1.
Arc-length 
LS-DYNA Theory Manual 
Another problem is that the feasible and infeasible solution may be too close to the last 
converged solution, making the result from the simulation very unpredictable.  For this 
a  parameter  𝛼  is  introduced  that  translates  the  center  of  the  spatial  sphere  in  the 
direction  of  the  linear  prediction  (i.e.,  the  first  Newton  iterate  of  the  implicit  solution 
procedure).  Assuming that this prediction is in the direction we want, using 𝛼 < 0 will 
move the center, and consequently the infeasible solution, away from where the iterates 
are taking place.  In addition, the radius of the arc will increase making it less probable 
to find the incorrect solution.  This option has shown effective in solving snap-through 
problems when using small steps to resolve maximum load values, and is illustrated in 
figures (g) and (h).  For snap-back problems, using 𝛼 = 1 could be an interesting choice 
since  this  centers  the  arc  right  between  the  previously  converged  point  and  the  first 
predictor  in  the  arc  length  method,  thus  encouraging  the  next  solution  to  be  found  in 
the reversed direction.  An example of a snap-back problem is shown in Figure 38-3. 
38.2  Nonlinear equations 
The  following,  except  for  a  change  in  notation,  is  very  similar  to  the  nonlinear  theory 
presented in the previous chapter.  The generalization is that 𝑡 will here be treated as an 
independent  variable  that  is  constrained  by  arc-length  instead  of  given  as  a  constant.  
The nonlinear variables are denoted 
𝒙 = [
𝒙𝐼
𝒙𝐷
],
(38.1)
that  we  assume  can  be  divided  into  a  set  of  independent  and  dependent  variables.  
Furthermore  we  have  the  time  parameter  𝑡  which  may  serve  as  the  actual  time  (for 
dynamic  problems)  or  just  a  stepping  parameter  (for  quasi-static  problems).    The 
division  into  independent  and  dependent  variables  is  motivated  by  the  constraint 
equation that must be fulfilled, i.e., 
From the constraint, the constraint matrix is evaluated as 
𝒉(𝒙, 𝑡) = 𝒉(𝒙𝐼, 𝒙𝐷, 𝑡) = 𝟎.
𝜕𝒉
𝜕𝒙
= [
𝜕𝒉
𝜕𝒙𝐼
𝜕𝒉
𝜕𝒙𝐷
] = [𝑪𝐷𝐼 𝑪𝐷𝐷],
(38.2)
(38.3)
which  in  turn  determines  the  space  of  trial  functions  used  to  establish  the  nonlinear 
finite element equation,  
[𝑰𝐼𝐼 −(𝑪𝐷𝐷
−1 𝑪𝐷𝐼)
𝑇][
𝒓𝐼
𝒓𝐷
] = 𝟎,
where  
𝒓(𝒙, 𝑡) = 𝒓(𝒙𝐼, 𝒙𝐷, 𝑡) = [
𝒓𝐼
𝒓𝐷
]
(38.4)
(38.5)
is  the  full  residual  divided  into  the  set  of  independent  and  dependent  variables.    See 
previous chapter for further details leading up to (38.4).
LS-DYNA Theory Manual 
Arc-length 
38.3  Newton iterations 
Here we assume that we are in a given configuration given by 
𝒙(𝑛,𝑖) = 𝒙(𝑛) + ∆𝒙(𝑛,𝑖),
𝑡(𝑛,𝑖) = 𝑡(𝑛) + ∆𝑡(𝑛,𝑖).
(38.6)
where  superscript  𝑛 = 0, 1, 2, …  represents  converged  implicit  states  and  𝑖 = 0, 1, 2, … 
represents  non-converged  Newton  iterates.    We  implicitly  assume  that  𝒙(0) = 𝒙̅, 
∆𝒙(𝑛,0) = 𝟎, 𝑡(0) = 0 and ∆𝑡(𝑛,0) = 0 are given.  In this configuration LS-DYNA computes 
the full residual given as 
as well as its dependence on the time parameter 
𝒓(𝑛,𝑖) = [
𝒓𝐼
𝒓𝐷
],
(𝑛,𝑖)
)
=
(
𝜕𝒓
𝜕𝑡
𝜕𝒓𝐼
⎤
⎡
𝜕𝑡
⎥⎥⎥
⎢⎢⎢
, 
𝜕𝒓𝐷
𝜕𝑡 ⎦
⎣
together with the stiffness matrix given as 
(𝑛,𝑖)
)
= [
(
𝜕𝒓
𝜕𝒙
𝑲𝐼𝐼 𝑲𝐼𝐷
𝑲𝐷𝐼 𝑲𝐷𝐷
].
(38.7)
(38.8)
(38.9)
Likewise  the  constraint  residual,  its  dependence  on  the  time  parameter  and  constraint 
matrix are evaluated and given by 
𝒉(𝑛,𝑖) = 𝒉,
(𝑛,𝑖)
𝜕𝒉
𝜕𝑡
, 
)
=
(𝑛,𝑖)
(
(
𝜕𝒉
𝜕𝑡
𝜕𝒉
𝜕𝒙
)
= [𝑪𝐷𝐼 𝑪𝐷𝐷].
The reduced residual and stiffness matrix are then formed as 
𝑲̂𝐼𝐼 = [𝑰𝐼𝐼 −(𝑪𝐷𝐷
−1 𝑪𝐷𝐼)
𝑇] [
𝒓 ̂𝐼 = [𝑰𝐼𝐼 −(𝑪𝐷𝐷
−1 𝑪𝐷𝐼)
𝑇] {[
𝜕𝒓 ̂𝐼
𝜕𝑡
= [𝑰𝐼𝐼 −(𝑪𝐷𝐷
−1 𝑪𝐷𝐼)
𝑇]
] − [
𝑲𝐼𝐼 𝑲𝐼𝐷
𝑲𝐷𝐼 𝑲𝐷𝐷
𝒓𝐼
𝑲𝐼𝐷
𝒓𝐷
𝑲𝐷𝐷
⎧
{{
⎨
{{
⎩
𝜕𝒓𝐼
⎤
⎡
𝜕𝑡
⎥⎥⎥
⎢⎢⎢
𝜕𝒓𝐷
𝜕𝑡 ⎦
⎣
− [
] [
𝑰𝐼𝐼
−1 𝑪𝐷𝐼
−𝑪𝐷𝐷
−1 𝒉} , 
] 𝑪𝐷𝐷
] , 
𝑲𝐼𝐷
𝑲𝐷𝐷
] 𝑪𝐷𝐷
−1 𝜕𝒉
𝜕𝑡
⎫
}}
⎬
}}
⎭
, 
(38.10)
(38.11)
and the independent search direction is given by 
𝛿𝒙𝐼 = 𝑠𝛿𝒙𝐼
𝑠 + 𝛿𝑡
𝜕𝒙𝐼
𝜕𝑡
.
LS-DYNA Draft
Arc-length 
LS-DYNA Theory Manual 
Here 𝑠 is the line search parameter and 
𝑠 = −𝑲̂𝐼𝐼
𝛿𝒙𝐼
𝜕𝒙𝐼
= −𝑲̂𝐼𝐼
𝜕𝑡
−1𝒓 ̂𝐼,
−1 𝜕𝒓 ̂𝐼
𝜕𝑡
.
The full search direction is completed by computing the dependent part as 
𝛿𝒙𝐷 = 𝑠𝛿𝒙𝐷
𝑠 + 𝛿𝑡
𝜕𝒙𝐷
𝜕𝑡
,
where 
𝑠 = −𝑪𝐷𝐷
𝛿𝒙𝐷
𝜕𝒙𝐷
𝜕𝑡
Finally the new configuration is updated by means of 
𝑠 − 𝑪𝐷𝐷
−1 𝑪𝐷𝐼𝛿𝒙𝐼
𝜕𝒙𝐼
−1 𝑪𝐷𝐼
𝜕𝑡
−1 𝒉,
−1 𝜕𝒉
𝜕𝑡
= −𝑪𝐷𝐷
− 𝑪𝐷𝐷
.
(𝑛,𝑖+1) = ∆𝒙𝐼
(𝑛,𝑖+1) = ∆𝒙𝐷
∆𝒙𝐼
∆𝒙𝐷
∆𝑡(𝑛,𝑖+1) = ∆𝑡(𝑛,𝑖) + 𝛿𝑡.
(𝑛,𝑖) + 𝛿𝒙𝐼,
(𝑛,𝑖) + 𝛿𝒙𝐷, 
Upon convergence we set 
and hence 
(𝑛,𝑖+1),
(𝑛) = ∆𝒙𝐼
∆𝒙𝐼
(𝑛,𝑖+1), 
(𝑛) = ∆𝒙𝐷
∆𝒙𝐷
∆𝑡(𝑛) = ∆𝑡(𝑛,𝑖+1),
(𝑛) + ∆𝒙𝐼
(𝑛+1) = 𝒙𝐼
𝒙𝐼
(𝑛) + ∆𝒙𝐷
(𝑛+1) = 𝒙𝐷
𝒙𝐷
𝑡(𝑛+1) = 𝑡(𝑛) + ∆𝑡(𝑛).
(𝑛) ,
(𝑛), 
(38.13)
(38.14)
(38.15)
(38.16)
(38.17)
(38.18)
LS-DYNA Theory Manual 
Arc-length 
Previously converged solution
Infeasible solution
Feasible solution
Predictore solution, found in the outward
Normal direction of previous arc
Infeasible predictor solution
Corrector steps occur along the arc
Figure 38.2.  Predictor and corrector steps 
38.4  Arc-length constraint – predictor step 
For the predictor step, 𝑖 = 0, the following constraint is imposed 
(1 − 𝜓)
(𝑛,1))
(∆𝒙𝐼
(0,1))
(∆𝒙𝐼
(𝑛,1)
∆𝒙𝐼
(0,1)
∆𝒙𝐼
+ 𝜓
∆𝑡(𝑛,1)∆𝑡(𝑛,1)
∆𝑡(0,1)∆𝑡(0,1) − 1 = 0, 
where for 𝑛 = 0 we use 
(0,1) = ∆𝑡 ̅
∆𝒙𝐼
∆𝑡(0,1) = ∆𝑡 ̅. 
𝜕𝒙𝐼
𝜕𝑡
(38.19)
(38.20)
Arc-length 
LS-DYNA Theory Manual 
Referring to Figure 38.2 this constraint is geometrically interpreted as to find a predictor 
solution on the arc with the previously converged solution as its center.  Writing out the 
above in terms of known quantities results in the following two possible values of the 
increment in time step parameter 
𝛿𝑡± = ±
𝜕𝒙𝐼
𝜕𝑡
𝑇 𝜕𝒙𝐼
𝜕𝑡
)
⎜⎛𝜓𝑥 (
⎝
+ 𝜓𝑡
⎟⎞
⎠
−1/2
,
corresponding to the two possible predictor solutions on the arc, where 
𝜓𝑥 =
𝜓𝑡 =
,
1 − 𝜓
(0,1))
∆𝒙𝐼
(∆𝒙𝐼
∆𝑡(0,1)∆𝑡(0,1).
(0,1)
(38.21)
(38.22)
The actual value used is detemined from the sign of 
𝑇 𝜕𝒙𝐼
𝜕𝑡
(𝑛−1,1))
(𝑛−1) −
2 (∆𝒙𝐼
∆𝒙𝐼
𝜓𝑥
(1 − 𝛼
)
+ 𝜓𝑡∆𝑡(𝑛−1), 
(38.23)
if positive 𝛿𝑡 = 𝛿𝑡+, otherwise 𝛿𝑡 = 𝛿𝑡−.  This condition is to say that the solution 
continues in the direction of the previously converged state, for the initial step 𝑛 = 0, 
𝛿𝑡 = 𝛿𝑡+. Again referring to Figure 38.2 we simply want to avoid going backwards to the 
infeasible predictor solution. 
38.5  Arc-length constraint – corrector steps 
For the corrector steps, 𝑖 > 0, the following constraint is imposed 
(1 − 𝜓)
(∆𝒙𝐼
(𝑛,𝑖+1) − 𝛼
∆𝒙𝐼
(1 − 𝛼
)
(𝑛,1))
(∆𝒙𝐼
(0,1))
(𝑛,𝑖+1) − 𝛼
(0,1)
∆𝒙𝐼
(∆𝒙𝐼
(𝑛,1))
∆𝒙𝐼
+ 𝜓
∆𝑡(𝑛,𝑖+1)∆𝑡(𝑛,𝑖+1)
∆𝑡(0,1)∆𝑡(0,1) − 1 = 0,  (38.24)
which  geometrically  says  that  we  should  find  the  next  iterate  on  the  arc.    Expanding, 
this amounts to 
(𝑛,𝑖) + 𝑠𝛿𝒙𝐼
𝛼𝑥 (∆𝒙𝐼
𝛼𝑡(∆𝑡(𝑛,𝑖) + 𝛿𝑡)(∆𝑡(𝑛,𝑖) + 𝛿𝑡) − 1 = 0,
𝑠 + 𝛿𝑡
∆𝒙𝐼
−
(𝑛,1))
𝜕𝒙𝐼
𝜕𝑡
(∆𝒙𝐼
(𝑛,𝑖) + 𝑠𝛿𝒙𝐼
𝑠 + 𝛿𝑡
𝜕𝒙𝐼
𝜕𝑡
−
(𝑛,1)) + 
∆𝒙𝐼
(38.25)
where 
𝛼𝑥 =
𝛼𝑡 =
1 − 𝜓
(0,1))
)
(1 − 𝛼
(∆𝒙𝐼
∆𝑡(0,1)∆𝑡(0,1).
(0,1)
∆𝒙𝐼
(38.26)
LS-DYNA Theory Manual 
Arc-length 
This can be written in terms of a polynomial in 𝑠 and 𝛿𝑡 as 
𝑎𝑠𝑠𝑠2 + 𝑎𝑡𝑡𝛿𝑡2 + 2𝑎𝑠𝑡𝑠𝛿𝑡 + 2𝑎𝑠𝑠 + 2𝑎𝑡𝛿𝑡
where 
+ 𝛼𝑡 
)
𝑎𝑡𝑡 = 𝛼𝑥 (
𝑠)𝑇𝛿𝒙𝐼
𝑎𝑠𝑠 = 𝛼𝑥 (𝛿𝒙𝐼
𝑇 𝜕𝒙𝐼
𝜕𝒙𝐼
𝜕𝑡
𝜕𝑡
𝑠)𝑇 𝜕𝒙𝐼
𝜕𝑡
𝑠)𝑇 𝜕𝒙𝐼
𝜕𝑡
(𝑛,𝑖) −
𝑎𝑠𝑡 = 𝛼𝑥(𝛿𝒙𝐼
𝑎𝑠𝑡 = 𝛼𝑥(𝛿𝒙𝐼
𝑎𝑠 = 𝛼𝑥 (∆𝒙𝐼
𝑎𝑡 = 𝛼𝑥 (∆𝒙𝐼
(𝑛,𝑖) −
(𝑛,1))
∆𝒙𝐼
+ 𝛼𝑡∆𝑡(𝑛,𝑖).
(𝑛,1))
∆𝒙𝐼
𝑠 
𝛿𝒙𝐼
𝑇 𝜕𝒙𝐼
𝜕𝑡
(38.27)
(38.28)
For  a  given  line  search  parameter  value,  the  time  increment  can  have  two  possible 
values 
𝛿𝑡± =
−𝑎𝑠𝑡𝑠 − 𝑎𝑡 ± √(𝑎𝑠𝑡
2 − 𝑎𝑡𝑡𝑎𝑠𝑠)𝑠2 + 2(𝑎𝑠𝑡𝑎𝑡 − 𝑎𝑠𝑎𝑡𝑡)𝑠 + 𝑎𝑡
. 
(38.29)
𝑎𝑡𝑡
and  the  value  we  use  for  the  update  is  given  by  𝛿𝑡 = 𝛿𝑡+  if  𝑎𝑡 ≥ 0,  otherwise  𝛿𝑡 = 𝛿𝑡−.  
This decision is based on the requirement of having 𝛿𝑡 → 0 when 𝑠 → 0.
Arc-length 
LS-DYNA Theory Manual 
Panel Response
 1
 0.8
 0.6
 0.4
 0.2
 0
 0
 0.2
 0.4
 0.6
 0.8
 1
 1.2
 1.4
Displacement
Figure 38-3 Snap-back buckling of panel, normalized force displacement 
curve shown
LS-DYNA Theory Manual 
Sparse Direct Linear Equation Solvers 
39    
Sparse Direct Linear Equation Solvers 
LS-DYNA  has  5  options  for  direct  solution  of  the  sparse  systems  of  linear 
equations that arise in LS-DYNA.  All 5 options are based on the multifrontal algorithm 
[Duff  and  Reid,  1983].    Multifrontal  is  a  member  of  the  current  generation  of  sparsity 
preserving factorization algorithms that also have very fast computational rates.  That is 
multifrontal works with a sparsity preserving ordering to reduce the overall size of the 
direct factorization and the amount of work it takes to compute that factorization. 
39.1  Sparsity Preserving Orderings 
In LS-DYNA there are two ordering algorithms for preserving the sparsity of the 
direct factorization.  The algorithms are Multiple Minimum Degree (MMD) and METIS 
[Karypis and Kumar, 1998].  MMD computes the ordering using locally based decisions 
and a bottom-up approach.  It is inexpensive and very effective for small problems that 
are problems with fewer than 100,000 rows.  METIS computes the ordering from a top 
down  approach.    While  METIS  usually  takes  more  time  than  MMD  to  compute  the 
ordering, the METIS ordering reduces the work for the factorization enough to recover 
the additional ordering cost.  METIS is especially effective for large problems, especially 
those that are modeling three-dimensional solids.    
The  user  can  specify  either  algorithm  using  keyword  *CONTROL_IMPLICIT_-
LINEAR.    The  default  is  to  use  MMD  for problems  with  fewer  than  100,000  rows  and 
METIS  for  problems  with  more  than  100,000  rows.    We  recommend  that  the  user  try 
both orderings as sometimes MMD is better than METIS on large problems that are not 
three-dimensional solids.
Sparse Direct Linear Equation Solvers 
LS-DYNA Theory Manual 
39.2  Multifrontal Algorithm 
The  multifrontal  algorithm  factors  a  sparse  matrix  in  a  way  that  vastly  reduces 
the amount of work required to compute the factorization compared to methods such as 
the  frontal,  profile,  skyline,  and  variable  band.    These  older  methods  counted  on 
clustering the nonzero entries of the factorization close to the diagonal to keep the size 
of the factorization and the amount of work required to compute the factorization to a 
minimum.    The  factorization  was  then  computed  in  a  serial,  left-to-right  fashion, 
essentially following a chain of computations.   
The multifrontal algorithm instead follows a tree of computations where the tree 
structure is established by the sparsity preserving orderings, See Figure 39.1.  It is this 
tree structure that greatly reduces the work required to compute a factorization and the 
size  of  the  resulting  factorization.    At  the  bottom  of  the  tree,  a  frontal  matrix  is 
assembled with the original matrix data and those columns that are fully assembled are 
eliminated.  The remainder of the frontal matrix is updated from the factored columns 
and  passed  up  the  tree  to the  parent  front  in  what  is  called  an  update  matrix.    As  the 
computation  works  its  way  up  the  tree,  a  frontal  matrix  is  formed  by  assembling  the 
original  matrix  data  and  the  update  matrices  from  its  children  in  the  tree.    The  fully 
assembled columns are factored and the remaining columns updated and passed up the 
tree.  At the root (top) of the tree, the remaining columns are factored.  
By  organizing  the  factorization  as  a  sequence  of  partial  factorization  of  dense 
frontal matrices, the multifrontal algorithm can be very fast in performing the required 
computations.    It  can  use  all  of  the  modern  technology  for  dense  linear  algebra  to  get 
high performance computational kernels that should achieve near peak computational 
performance  for  a  given  processor.    Only  1%  to  5%  of  the  work  of  the  factorization  is 
performed with slower operations such as scatter/gather.
LS-DYNA Theory Manual 
Sparse Direct Linear Equation Solvers 
original matrix data
From children fronts
To parent front
computations in single front
Figure 39.2.  Single front algorithm. 
39.3  The Five Solver Options  
In  LS-DYNA  three  new  direct  solution  options  were  added.    For  backward 
compatibility, the two older options were kept.  The five options are: 
Multifrontal elimination tree
Figure 39.1.  Multifrontal algorithm. 
Solver   Method
Sparse Direct Linear Equation Solvers 
LS-DYNA Theory Manual 
No. 
1 
3 
4 
5 
6 
Older  implementaion  of  Solver  No.    4.    Uses  Real*4  arithmetic,  has  out  of 
memory  capabilities  as  well  as  distributed  memory  parallelism.    Only  uses 
MMD  ordering.    Was  former  default  method.    Retained  for  backward 
compatibility.    We  recommend  switching  to  Solver  No.    4  for  improved 
performance. 
Same as 1 except uses Real*8 arithmetic.  We recommend switching to Solver 
No.  5 or 6 for improved performance. 
Real*4  implementation  of  multifrontal  which  includes  automatic  out-of-
memory  capabilities  as  well  as  distributed  memory  parallelism.    Can  use 
either MMD or METIS orderings.  Default method. 
Real*8 implementation of Solver No.  4. 
Multifrontal solver from BCSLIB-EXT [Boeing Company, 1999].  Uses Real*8 
arithmetic  with  extensive  capabilities  for  large  problems  and  some  Shared 
Memory Parallelism. 
Can use either MMD or METIS orderings.  If the other solvers cannot factor 
the problem in the allocated memory, try using this solver. 
We strongly recommend using Solvers 4 through 6.  Solvers 1 and 3 are included 
for backward compatibility with older versions of LS-DYNA but are slower the Solvers 
4 through 6.  Solvers 4 and 5 are 2 to 6 times faster than the older versions, respectively.  
Solver 6 on a single processor computer should be comparable to Solver 5 but has more 
extensive capabilities for solving very large problems with limited memory.  Solvers 4 
and  5  should  be  used  for  distributed  memory  parallel  implementations  of  LS-DYNA.  
Solver 6 can be used in shared memory parallel. 
In an installation of LS-DYNA where both integer and real numbers are stored in 
8 byte quantities, then Solvers 1 and 3 are equivalent and Solvers 4 and 5 are equivalent. 
39.4  Treating Matrix Singularities 
LS-DYNA  has  two  different  techniques  for  preventing  singularities  in  the 
stiffness matrix, K.  The most common type of matrix singularity arises from the use of 
certain types of shell elements.  These shell elements generate no matrix contribution in 
the normal direction for each node.  Depending on the geometry around the node and 
what  other  types  of  elements  are  connected  to  the  node,  there  may  or  may  not  be  a 
matrix  singularity  associated  with  the  rotation  around  the  normal  direction  at  one  or 
more nodes.  This is commonly called the drilling rotation singularity.   
The first way LS-DYNA has for preventing such matrix singularities is to add a 
small  amount  of  stiffness  in  the  normal  direction  at  each  node  of  every  shell  element 
that has the drilling rotation problem.  This “drilling” stiffness matrix is orthogonal to
LS-DYNA Theory Manual 
Sparse Direct Linear Equation Solvers 
rigid body motions.  The user can control whether this approach is used and how much 
stiffness is added via the *CONTROL_IMPLICIT_SOLUTION keyword card.  DRLMTH 
and  DRLPARM  are  set  in  fields  5  and  6.    If  DRLMTH = 1  then  this  approach  is  used.  
The amount of stiffness added is controlled via DRLPARM.  The default for DRLPARM 
is 1.0 for linear problems and 100.0 for nonlinear problems.  DRLPARM ∗ .0001 is added 
in the normal direction at each node to the diagonal terms associated with the rotational 
degrees  of  freedom  for  certain  types  of  elemental  matrices.    For  eigenvalue  problems 
the amount of stiffness added is 1.E-12. 
Adding  stiffness  to  handle  the  drilling  rotation  problem  has  been  used 
extensively.    While  a  robust  and  reliable  approach,  its  drawback  is  that  the  added 
stiffness may affect the quality of the computed results.  The user can also select not to 
use  this  approach  and  depend  solely  on  AUTOSPC,  the  other  method  for  preventing 
matrix singularities. 
AUTOSPC  stands  for  AUTOmatic  Single  Point  Constraints.      AUTOSPC 
examines  K  after  all  of  the  elemental  matrices  have  been  assembled  and  all  of  the 
constraints  have  been  applied  for  columns  that  are  singular.    The  user  controls  AU-
TOSPC using ASPCMTH and ASPCTOL, fields 7 and 8 of the CONTROL_IMPLICIT_-
SOLUTION  keyword  card.    If  ASPCMTH = 1,  AUTOSPC  is  used.    For  every  set  of 
columns of K that correspond to the translational or rotational degrees of freedom for a 
node  or  rigid  body  those  columns  are  examined.    The  singular  values  of  the  diagonal 
block  of  the  columns  are  computed.    If  the  ratio  of  the  smallest  and  largest  singular 
values  is  less  than  ASPCTOL  then  the  set  of  the  columns  is  declared  singular  and  a 
constraint  is  imposed  to  remove  the  singularity.    The  defaults  for  ASPCTOL  is  1.E-6 
when  the  matrix  is  assembled  in  REAL*4  precision  and  1.E-8  when  REAL*8  is  used.  
The  imposed  constraint  sets  the  degree  of  freedom  to  zero  that  is  associated  with  the 
column  that  has  the  largest  component  in  the  null  space  of  the  columns.    If  all  of  the 
singular  values  are  less  than  ASPCTOL  all  of  the  degrees  of  freedom  in  the  block  are 
constrained to zero.
LS-DYNA Theory Manual 
Sparse Eigensolver 
40    
Sparse Eigensolver 
LS-DYNA  now  includes  the  Block  Shift  and  Invert  Lanczos  eigensolver  from 
BCSLIB-EXT.  This eigensolver is used in LS-DYNA to compute the normal modes and 
mode shapes for the vibration analysis problem 
where  𝐊  and  𝐌are  the  assembled  stiffness  and  mass  matrices,  𝚽  are  the  eigenvectors 
(normal mode shapes) and 𝚲 are the eigenvalues (normal modes).   
𝐊𝚽 = 𝐌𝚽𝚲,
(40.1)
The Lanczos algorithm iteratively computes a better and better approximation to 
the extreme eigenvalues and the corresponding eigenvectors of the ordinary eigenvalue 
problem  𝐀𝚽 = 𝚽𝚲where  𝐀  is  a  real  symmetric  matrix  using  only  matrix-vector 
multiplies.  To use Lanczos on the vibration analysis problem it must be changed to 
(𝐊 − 𝛔𝐌)−1𝐌𝚽 = 𝚽𝚯,
(40.2)
where each shifted and inverted eigenvalue 𝜃𝑖 = 1/(𝜆𝑖 − 𝜎).  This change to an ordinary 
eigenvalue  problem  makes  the  eigenvalues  of  the  original  problem  near  σ  become the 
extreme  eigenvalues  of  the  ordinary  eigenvalue  problem.    This  helps  the  Lanczos 
algorithm compute those eigenvalues quickly.   
BCSLIB-EXT  uses  a  sophisticated  logic  to  choose  a  sequence  of  shifts,  𝜎𝑖,  to 
enable  the  computation  of  a  large  number  of  eigenvalues  and  eigenvectors.    At  each 
shift  the  factorization  of  𝐊 − 𝛔𝐌  is  computed.    The  factorization  provides  the  matrix 
inertia  that  tells  the  algorithm  how  many  eigenvalues  are  to  the  left  of  any  given  𝜎𝑖.  
Given  the  inertia  information,  BCSLIB-EXT  can  tell  how  many  eigenvalues  are  in  a 
given  interval  and  determine  if  all  of  the  eigenvalues  in  that  interval  have  been 
computed.  As a result, BCSLIB-EXT is a very robust eigensolver. 
The  implementation  of  BCSLIB-EXT  in  LS-DYNA  includes  a  shared  memory 
implementation.      However  only  limited  parallel  speed-up  is  available  for  most 
problems.    This  is  because  the  eigensolution  requires  a  vast  amount  of  data  that  for 
most  problems  this  data  has  to  be  stored  on  I/O  files.    The  wall  clock  time  for  the
Sparse Eigensolver 
LS-DYNA Theory Manual 
eigensolver is as much a function of the speed of the I/O subsystem on the computer as 
the CPU time.  Parallelism can only speed up the CPU time and does nothing to speed-
up the I/O time.   
The  user  can  request  how  many  and  which  eigenvalues  to  compute  using  the 
keyword *CONTROL_IMPLICIT_EIGENVALUE.  Via the parameters on this keyword, 
the user can request any of the following problems: 
•  Compute the lowest 50 modes (that is nearest to zero) 
•  Compute the 20 modes nearest to 30 Hz. 
•  Compute the lowest 20 modes between 10 Hz and 50 Hz. 
•  Compute all of the modes between 10 Hz and 50 Hz. 
•  Compute all of the modes below 50 Hz. 
•  Compute the 30 modes nearest to 30 Hz between 10 Hz and 50 Hz. 
40.1  The Eigenvalue Problem for Rotating Systems 
Rotating  systems,  such  as  the  compressor  and  turbine  assembly  of  a  jet  engine, 
have  large  inertial  forces  that  are  functions  of  the  distance  from  the  axis  of  rotation.  
These forces are naturally generated in LS-DYNA if the system is modeled as rotating at 
the  proper  angular  velocity.    However,  this  is  often  inconvenient  for  postprocessing 
because  the  solution  has  an  oscillatory  character  imposed  it  due  to  the  rotation.    A 
commonly  used  approach  to  bypass  this  difficulty  is  to  impose  body  forces  that  are 
equivalent to the inertial forces due to rotation.  In LS-DYNA, these forces are imposed 
through *LOAD_BODY_GENERALIZED and related keywords. 
For a system with a constant angular velocity 𝛚 = {𝜔𝑥, 𝜔𝑦, 𝜔𝑧}T, the body force 
added to the applied load is  
𝐅B = −𝐌{2𝛚 × 𝐮̇ + 𝛚 × (𝛚 × (𝐫 + 𝐮))}.
(40.3)
In  this  equation, 𝐫  is  the  initial  coordinate  at a  point  and 𝐮  is  the  displacement.  
Because  the  body  force  is  a  function  of  both  the  velocity  and  displacement,  it 
contributes  both  damping  and  stiffness  matrices  to  the  eigenvalue  problem.  
Furthermore,  since  the  term  involving  the  initial  coordinate  creates  an  initial  stress  in 
the  structure,  the  initial  stress  matrix  𝐊𝜎  (also  called  the  nonlinear  stiffness)  is  also 
added to the eigenvalue problem.
LS-DYNA Theory Manual 
Sparse Eigensolver 
The damping and stiffness terms are easily derived in matrix form once the cross 
product is expressed in matrix form.  
𝛚 × 𝐫 = 𝛀𝐫 =
⎡
𝜔𝑧
⎢⎢
−𝜔𝑦 𝜔𝑥
⎣
−𝜔𝑧 𝜔𝑦
⎤
−𝜔𝑥
⎥⎥
0 ⎦
{
}. 
The linearized equation for vibration is 
𝐌𝐮̈ + 𝐂𝐮̇ + [𝐊 + 𝐊σ]𝐮 = −𝐌{𝛀𝐮̇ + 𝛀2𝐮}.
(40.4)
(40.5)
Rewriting  this  equation  into  the  traditional  form  for  eigenvalue  analysis 
produces: 
𝐌𝐮̈ + 𝐂R𝐮̇ + 𝐊R𝐮 = 0
𝐂R = 𝐂 + 𝐌𝛀 
𝐌𝐮̈ + 𝐂R𝐮̇ + 𝐊R𝐮 = 0.
(40.6)
The  inertial  contribution  to  the  damping  matrix  is  not  symmetric,  nor  does  it 
fulfill the requirements for Rayleigh damping, and therefore the resulting eigenvectors 
and  eigenvalues  are  complex.    The  inertial  term  to  the  stiffness  matrix  is,  however, 
symmetric and it softens the structure, thereby reducing its natural frequencies.  
If  the  damping  term  is  omitted,  the  matrices  are  real  and  symmetric,  and  the 
resulting  eigenvalue  problem  may  be  solved  with  the  standard  eigenvalue  methods.  
The  natural  frequencies  won’t  be  correct,  but  they  are  typically  close  enough  to  the 
complex solution that they can be used for initial design calculations.
LS-DYNA Theory Manual 
Boundary Element Method 
41    
Boundary Element Method 
LS-DYNA can be used to solve for the steady state or transient fluid flow about a 
body using a boundary element method.  The method is based on the work of Maskew 
[1987],  with  the  extension  to  unsteady  flow  with  arbitrary  body  motion  following  the 
work of Katz and Maskew [1988].  The theory which underlies the method is restricted 
to  inviscid,  incompressible,  attached  fluid  flow.    The  method  should  not  be  used  to 
analyze flows where shocks or cavitation are present.   
In practice the method can be successfully applied to a wider class of fluid flow 
problems than the assumption of inviscid, incompressible, attached flow would imply.  
Many flows of practical engineering significance have large Reynolds numbers (above 1 
million).    For  these  flows  the  effects  of  fluid  viscosity  are  small  if  the  flow  remains 
attached, and the assumption of zero viscosity may not be a significant limitation.  Flow 
separation does not necessarily invalidate the analysis.  If well-defined separation lines 
exist on the body, then wakes can be attached to these separation lines and reasonable 
results  can  be  obtained.    The  Prandtl-Glauert  rule  can  be  used  to  correct  for  non-zero 
Mach  numbers  in  air,  so  the  effects  of  aerodynamic  compressibility  can  be  correctly 
modeled (as long as no shocks are present). 
41.1  Governing Equations 
The partial differential equation governing inviscid, incompressible fluid flow is 
given by LaPlace’s equation 
∇2𝛷 = 0,
(41.1)
where 𝛷 is the velocity potential (a scalar function).  The fluid velocity anywhere in the 
flow  field  is  equal  to  the  gradient  of  𝛷.    The  boundary  condition  on  this  partial 
differntial  equation  is  provided  by  the  condition  that  there  must  be  no  flow  in  the 
direction normal to the surface of the body.  Note that time does not appear in Equation
Boundary Element Method 
LS-DYNA Theory Manual 
(41.1).    This  is  because  the  assumption  of  incompressibility  implies  an  infinite  sound 
speed; any disturbance is felt everywhere in the fluid instantaneously.  Although this is 
not  true  for  real  fluids,  it  is  a  valid  approximation  for  a  wide  class  of  low-speed  flow 
problems. 
Equation  (41.1)  is  solved  by  discretizing  the  surface  of  the  body  with  a  set  of 
quadrilateral or triangular surface segments (boundary elements).  Each segment has an 
associated  source  and  doublet  strength.    The  source  strengths  are  computed  from  the 
free-stream  velocity,  and  the  doublet  strengths  are  determined  from  the  boundary 
condition.  By requiring that the normal component of the fluid velocity be zero at the 
center of each surface segment, a linear system of equations is formed with the number 
of equations equal to the number of unknown doublet strengths.  When this system is 
solved, the doublet strengths are known.  The source and doublet distributions on the 
surface of the body then completely determine the flow everywhere in the fluid. 
The linear system for the unknown doublet strengths is shown in Equation (1.2). 
[mic]{𝜇} = {rhs}.
(41.2)
In  this  equation  μ  are  the  doublet  strengths,  [mic  is  the  matrix  of  influence 
coefficients which relate the doublet strength of a given segment to the normal velocity 
at another segment’s mid-point, and rhs is a right-hand-side vector computed from the 
known  source  strengths.    Note  that  mic  is  a  fully-populated  matrix.    Thus,  the  cost  to 
compute and store the matrix increases with the square of the number of segments used 
to discretize the surface of the body, while the cost to factor this matrix increases with 
the cube of the number of segments.  Users should keep these relations in mind when 
defining  the  surface  segments.    A  surface  of  1000  segments  can  be  easily  handled  on 
most any computer, but a 10,000 segment representation would not be feasible on any 
but the most powerful supercomputers. 
41.2  Surface Representation 
The surface of the body is discretized by a set of triagular or quadrilateral surface 
segments.  The best fluid-structure interaction results will be obtained if the boundary 
element  segments  coincide  with,  and  use  identical  nodes  as,  the  structural  segments 
used  to  define  the  body.    An  input  format  has  been  implemented  to  make  this  easy  if 
thin shell elements are used to define the structure .  Using the 
same  nodes  to  define  the  boundary  elements  and  the  structure  guarantees  that  the 
boundary  elements  follow  the  structure  as  it  deforms,  and  provides  a  means  for  the 
fluid pressure to load the structure.
LS-DYNA Theory Manual 
Boundary Element Method 
normal
node 4
node 3
node 1
node 2
Figure  41.1.    Counter-clockwise  ordering  of  nodes  when  viewed  from  fluid
looking towards solid provides unit normal vector pointing into the fluid. 
The nodes used to define the corners of the boundary element segments must be 
ordered to provide a normal vector which points into the fluid (Figure 41.1). 
Triangular  segments  are  specified  by  using  the  same  node  for  the  3rd  and  4th 
corner of the segment (the same convention used for shell elements in LS-DYNA).  Very 
large  segments  can  be  used  with  no  loss  of  accuracy  in  regions  of  the  flow  where  the 
velocity gradients are small.  The size of the elements should be reduced in areas where 
large  velocity  gradients  are  present.    Finite-precision  arithmetic  on  the  computer  will 
cause problems if the segment aspect ratios are extremely large (greater than 1000).  The 
most  accurate  results  will  be  obtained  if  the  segments  are  rectangular,  and  triangular 
segments should be avoided except for cases where they are absolutely required. 
The fluid velocities (and, therefore, the fluid 
41.3  The Neighbor Array  
pressures)  are  determined  by  the  gradient  of  the  velocity  potential.    On  the  surface  of 
the  body,  this  can  be  most  easily  computed  by  taking  derivatives  of  the  doublet 
distribution on the surface.  These derivatives are computed using the doublet strengths 
on the boundary element segments.  The “Neighbor Array” is used to specify how the 
gradient is computed  for each boundary element segment.  Thus,  accurate results will 
not be obtained unless the neighbor array is correctly specified by the user. 
Each  boundary  element  segment  has  4  sides  .    Side  1  connects 
the 1st and 2nd nodes, side 2 connects the 2nd and 3rd nodes, etc.  The 4th side is null 
for triangular segments.
Boundary Element Method 
LS-DYNA Theory Manual 
node 4
side 3
side 4
node 3
side 2
side 1
node 1
node 2
Figure 41.2.  Each segment has 4 sides. 
For  most  segments  the  specification  of  neighbors  is  straightforward.    For  the 
typical case a rectangular segment is surrounded by 4 other segments, and the neighbor 
array is as shown in Figure 41.3.  A biquadratic curve fit is computed, and the gradient 
is  computed  as  the  analytical  derivative  of  this  biquadratic  curve  fit  evaluated  at  the 
center of segment j. 
There are several situations which call for a different specification of the neighbor 
array.    For  example,  boundary  element  wakes  result  in  discontinuous  doublet 
distributions,  and  the  biquadratic  curve  fit  should  not  be  computed  across  a  wake.  
Figure 41.4 illustrates a situation where a wake is attached to side 2 of segment 𝑗.  For 
this  situation  two  options  exist.    If  neighbor  (2, 𝑗)  is  set  to  zero,  then  a  linear 
computation  of  the  gradient  in  the  side  2  to  side  4  direction  will  be  made  using  the 
difference between the doublet strengths on segment 𝑗 and segment neighbor (4, 𝑗).  By 
specifying  neighbor  (2, 𝑗)  as  a  negative  number  the  biquadratic  curve  fit  will  be 
retained.    The  curve  fit  will  use  segment  𝑗,  segment  neighbor  (4, 𝑗),  and  segment  –
neighbor  (2, 𝑗);  which  is  located  on  the  opposite  side  of  segment  neighbor  (4, 𝑗)  as 
segment 𝑗.  The derivative in the side 2 to side 4 direction is then analytically evaluated 
neighbor (3, j)
neighbor(4, j)
side 4
side 3
segment j
side 1
neighbor (2, j)
side 2
neighbor (1, j)
Figure 41.3.  Typical neighbor specification.
LS-DYNA Theory Manual 
Boundary Element Method 
-neighbor (2, j)
neighbor (4, j)
segment j
side 4
side 2
Figure 41.4.  If neighbor (2, 𝑗) is a negative number it is assumed to lie on the 
opposite side of neighbor (4, 𝑗) as segment 𝑗. 
at the center of segement j using the quadratic curve fit of the doublet strengths on the 
three segments shown. 
A final possibility is that no neighbors at all are available in the side 2 to side 4 
direction.  In this case both neighbor (2, 𝑗) and neighbor (4, 𝑗) can be set to zero, and the 
gradient in that direction will be assumed to be zero.  This option should be used with 
caution,  as  the  resulting  fluid  pressures  will  not  be  accurate  for  three-dimensional 
flows.    However,  this  option  is  occaisionally  useful  where  quasi-two  dimensional 
results are desired.  All of the above options apply to the side 1 to side 3 direction in the 
obvious ways. 
For triangular boundary element segments side 4 is null.  Gradients in the side 2 
to side 4 direction can be computed as described above by setting neighbor (4, 𝑗) to zero 
(for a linear derivative computation) or to a negative number (to use the segment on the 
other  side  of  neighbor  (2, 𝑗)  and  a  quadratic  curve  fit).    There  may  also  be  another 
triangular segment which can be used as neighbor (4, 𝑗) .
Boundary Element Method 
LS-DYNA Theory Manual 
41.4  Wakes 
Wakes should be attached to the boundary element segments at the trailing edge 
of  a  lifting  surface  (such  as  a  wing,  propeller  blade,  rudder,  or  diving  plane).    Wakes 
should also be attached to known separation lines (such as the sharp leading edge of a 
delata wing at high angles of attack).  Wakes are required for the correct computation of 
surface  pressures  for  these  situations.    As  described  above,  two  segments  on  opposite 
sides of a wake should never be used as neighbors.  Correct specification of the wakes is 
required for accurate results. 
Wakes  convect  with  the  free-stream  velocity.    The  number  of  segments  in  the 
wake is controlled by the user, and should be set to provide a total wake length equal to 
5-10 times the characteristic streamwise dimension of the surface to which the wake is 
attached.    For  example,  if  the  wake  is  attached  to  the  trailing  edge  of  a  wing  whose 
chord is 1, then the total length of the wake should at least 5, and there is little point in 
making it longer than 10.  Note that each wake segment has a streamwise length equal 
to the magnitude of the free stream velocity times the time increment between calls to 
the Boundary Element Method routine.  This time increment is the maximum of the LS-
DYNA  time  step  and  DTBEM  specified  on  Card  1  of  the  BEM  input.    The  influence 
coefficients  for  the  wake  segments  must  be  recomputed  for  each  call  to  the  Boundary 
Element  Method,  but  these  influence  coefficients  do  not  enter  into  the  matrix  of 
influence coefficients which must be factored. 
41.5  Execution Time Control 
The  Boundary  Element  Method  will  dominate  the  total  execution  time  of  a  LS-
DYNA calculation unless the parameters provided on Card 1 of the BEM input are used 
to  reduce  the  number  of  calls  to  the  BEM.    This  can  usually  be  done  with  no  loss  in 
neighbor(4, j)
segment j
side 2
Figure 41.5.  Sometimes another triangular boundary element segment can be
used as neighbor(4,j). 
accuracy since the characteristic time of the structural dynamics and the fluid flow are
LS-DYNA Theory Manual 
Boundary Element Method 
so  different.    For  example,  the  characteristic  time  in  LS-DYNA  is  given  by  the 
characteristic length of the smallest structural element divided by the speed of sound of 
the  material.    For  typical  problems  this  characteristic  time  might  be  on  the  order  of 
microseconds.  Since the fluid is assumed to be incompressible (infinite speed of sound), 
the characteristic time of the fluid flow is given by the streamwise length of the smallest 
surface  (e.g.  a  rudder)  divided  by  the  fluid  velocity.    For  typical  problems  this 
characteristic  time  might  be  on  the  order  of  milliseconds.    Thus,  for  this  example,  the 
boundary  element  method  could  be  called  only  once  for  every  1000  LS-DYNA 
iterations, saving an enormous amount of computer time. 
The  parameter  DTBEM  on  Card  1  of  the  BEM  input  is  used  to  control  the  time 
increment  between  calls  to  the  boundary  element  method.    The  fluid  pressures 
computed  during  the last  call  to  the  BEM  will  continue  to  be  used  for  subsequent  LS-
DYNA iterations until DTBEM has elapsed. 
A  further  reduction  in  execution  time  may  be  obtained  for  some  applications 
using the input parameter IUPBEM.  This parameter controls the number of calls to the 
BEM  routine  between  computation  (and  factorization)  of  the  matrix  of  influence 
coefficients (these are time-consuming procedures).  If the motion of the body is entirely 
rigid  body  motion  there  is  no  need  to  recompute  and  factor  the  matrix  of  influence 
coefficients, and the execution time of the BEM can be significantly reduced by setting 
IUPBEM to a very large number.  For situations where the motion of the body is largely 
rigid body motion with some structural deformation an intermediate value (e.g. 10) for 
IUPBEM can be used.  It is the user’s responsibility to verify the accuracy of calculations 
obtained with IUPBEM greater than 1. 
The  final  parameter  for  controlling  the  execution  time  of  the  boundary  element 
method  is  FARBEM.    The  routine  which  calculates  the  influence  coefficients  switches 
between an expensive near-field and an inexpensive far-field calculation depending on 
the distance from the boundary element segment to the point of interest.  FARBEM is a 
nondimensional parameter which determines where the far-field boundary lies.  Values 
of FARBEM of 5 and greater will provide the most accurate results, while values as low 
as 2 will provide slightly reduced accuracy with a 50% reduction in the time required to 
compute the matrix of influence coefficients. 
41.6  Free-Stream Flow 
The  free-stream  flow  is  specified  in  the  second  card  of  input.    The  free-stream 
velocity  is  assumed  to  be  uniform.    The  free-stream  static  pressure  is  assumed  to  be 
uniform, and can be used to load the structure for hydrostatic pressure.  If the structure 
has an internal pressure, the free-stream static pressure should be  set to the difference 
between  the  external  and  internal  static  pressures.    The  Mach  number  can  be  used  to
Boundary Element Method 
LS-DYNA Theory Manual 
correct  for  the  effect  of  compressibility  in  air  (as  long  as  no  shocks  are  present).  
Following the Prandtl-Glauert correction, the pressures due to fluid flow are increased 
as follows 
𝑑𝑝corrected =
𝑑𝑝uncorrected
√1 − 𝑀2
(41.3)
where  M  is  the  free-stream  Mach  number.    Note  that  this  correction  is  only  valid  for 
flows in a gas (it is not valid for flows in water).
LS-DYNA Theory Manual 
SPH 
42    
SPH 
Smoothed  Particle  Hydrodynamics  (SPH)  is  an  N-body  integration  scheme 
developed  by  Lucy,  Gingold  and  Monaghan  [1977].    The  method  was  developed  to 
avoid  the  limitations  of  mesh  tangling  encountered  in  extreme  deformation  problems 
with  the  finite  element  method.    The  main  difference  between  classical  methods  and 
SPH is the absence of a grid.  Therefore, the particles are the computational framework 
on  which  the  governing  equations  are  resolved.    This  new  model  requires  a  new 
calculation method, which is briefly explained in the following. 
42.1  SPH Formulation  
42.1.1  Definitions  
The particle approximation of a function is: 
Πℎ𝑓 (𝑥) = ∫ 𝑓 (𝑦)𝑊(𝑥 − 𝑦, ℎ)𝑑𝑦,
where 𝑊 is the kernel function. 
The Kernel function 𝑊 is defined using the function 𝜃 by the relation: 
𝑊(𝐱, ℎ) =
ℎ(𝐱)𝑑
𝜃(𝐱).
(42.1)
(42.2)
where  𝑑  is  the  number  of  space  dimensions  and  ℎ  is  the  so-called  smoothing  length 
which varies in time and in space. 
𝑊(𝐱, ℎ)  should  be  a  centrally  peaked  function.    The  most  common  smoothing 
kernel used by the SPH community is the cubic B-spline which is defined by choosing 𝜃 
as:
SPH 
LS-DYNA Theory Manual 
𝜃(𝑢) = 𝐶 ×
⎧
{{{
⎨
{{{
⎩
1 −
𝑢2 +
𝑢3 for |𝑢| ≤ 1
(2 − 𝑢)3            for  1 ≤ |𝑢| ≤ 2
for 2 < |𝑢|
(42.3)
where  C  is  a  constant  of  normalization  that  depends  on  the  number  of  space 
dimensions.   
The SPH method is based on a quadrature formula for moving particles ((𝐱𝑖(𝑡)) 
𝑖 ∈ {1. . 𝑁}, where 𝐱𝑖(𝑡) is the location of particle 𝑖, which moves along the velocity field 
v. 
The particle approximation of a function can now be defined by: 
Πℎ𝑓 (𝐱𝑖) = ∑ 𝑤𝑗𝑓 (𝐱𝑖)𝑊(𝐱𝑖 − 𝐱𝑗, ℎ)
,
𝑗=1
(42.4)
where  𝑤𝑗 =
proportionally to the divergence of the flow. 
𝑚𝑗
𝜌𝑗
  is  the  “weight”  of  the  particle.    The  weight  of  a  particle  varies 
The SPH formalism implies a derivative operator.  A particle approximation for 
the  derivative  operator  must  be  defined.      Before  giving  the  definition  of  this 
approximation, we define the gradient of a function as: 
∇𝑓 (𝑥) = ∇𝑓 (𝑥) − 𝑓 (𝑥)∇1(𝑥),
(42.5)
where 1 is the unit function. 
Starting  from  this  relation,  we  can  define  the  particle  approximation  to  the 
gradient of a function: 
Πℎ∇𝑓 (𝐱𝑖) = ∑
𝑗=1
𝑚𝑗
𝜌𝑗
,
[𝑓 (𝐱𝑗)𝐴𝑖𝑗 − 𝑓 (𝐱𝑖)𝐴𝑖𝑗]
(42.6)
where 𝐴𝑖𝑗 = 1
ℎ𝑑+1 𝜃′(
||𝐱𝑖−𝐱𝑗||
). 
We can also define the particle approximation of the partial derivative  ∂
∂𝑥𝛼: 
Πℎ(
∂𝑓
∂𝑥𝛼)(𝐱𝑖) = ∑ 𝑤𝑗
𝑗=1
𝑓 (𝐱𝑗𝐴𝛼(𝐱𝑖, 𝐱𝑗),
(42.7)
where  𝐀  is  the  operator  defined  by:  𝐀(𝐱𝑖, 𝐱𝑗) =
ℎ𝑑+1(𝐱𝑖,𝐱𝑗)
(𝐱𝑖−𝐱𝑗)
|∣𝐱𝑖−𝐱𝑗∣|
𝜃′ (
|∣𝐱𝑖−𝐱𝑗∣|
ℎ(𝐱𝑖,𝐱𝑗)),  𝐴𝛼  is  the 
component 𝛼 of the 𝐀 vector.
LS-DYNA Theory Manual 
42.1.2  Discrete Form of Conservation Equations  
We are looking for the solution of the equation: 
𝐿𝑣(𝜙) + div𝐅(𝐱, 𝑡, 𝜙) = 𝑆,
SPH 
(42.8)
where 𝜙 ∈   𝑅𝑑 is the unknown, 𝐅𝛽 with 𝛽 ∈ {1. . 𝑑} represents the conservation law and 
𝐿𝑣 is the transport operator defined by: 
𝐿𝑣: 𝜙 → 𝐿𝑣(𝜙) =
∂𝜙
∂𝑡
+ ∑
𝑙=1
∂(𝐯𝑙𝜙)
.
∂𝑥𝑙
(42.9)
The strong formulation approximation: 
In the search of the strong solution, the equation is kept at its initial formulation.  
The discrete form of this problem implies the definition of the operator of derivation 𝐷 
defined by: 
𝐷: 𝜙 → 𝐷𝜙(𝑥) = ∇𝜙(𝑥) − 𝜙(𝑥)∇1(𝑥).
The particle approximation of this operator is:   
𝐷ℎ𝜙(𝐱𝑖) = ∑ 𝑤𝑗(𝜙(𝐱𝑗) − 𝜙(𝐱𝑖))𝐴𝑖𝑗
,
𝑗=1
where 𝐴𝑖𝑗 is defined previously. 
(42.10)
(42.11)
Finally, the discrete form of the strong formulation is written: 
𝑑𝑡
(𝑤𝑖𝜙(𝐱𝑖)) + 𝑤𝑖𝐷ℎ𝐹(𝐱𝑖) = 𝑤𝑖𝑆(𝐱𝑖),
(42.12)
But  this  form  is  not  conservative;  therefore  the  strong  formulation  is  not  numerically 
acceptable.  Thus, we are compelled to use the weak form. 
The weak formulation approximation: 
In the weak formulation, the adjoint of the 𝐿𝑣 operator is used: 
∗: 𝜙 → 𝐿𝑣
𝐿𝑣
∗(𝜙) =
∂𝜙
∂𝑡
+ ∑ 𝑣𝑙
𝑙=1
∂𝜙
∂𝑥𝑙
.
(42.13)
The discrete form of this operator corresponds to the discrete formulation of the adjoint 
of 𝐷ℎ,𝑠: 
𝐷ℎ,𝑠
∗ 𝜙(𝐱𝑖) = ∑ 𝑤𝑗(𝜙(𝐱𝑖
𝑗=1
)𝐴𝑖𝑗 − 𝜙(𝐱𝑗)𝐴𝑗𝑖).
(42.14)
A  discrete  adjoint  operator  for  the  partial  derivative  is  also  necessary,  and  is 
taken to be the 𝛼 − 𝑡ℎ component of the operator:
SPH 
LS-DYNA Theory Manual 
𝐷𝛼
∗𝜙(𝐱𝑖) = ∑ 𝑤𝑗
𝜙(𝐱𝑗)𝐴𝛼(𝐱𝑖, 𝐱𝑗) − 𝑤𝑗𝜙(𝐱𝑖)𝐴𝛼(𝐱𝑗, 𝐱𝑖)
(42.15)
𝑗=1
These  definitions  are  leading  to  a  conservative  method.    Hence,  all  the  conservative 
equations encountered in the SPH method will be solved using the weak form. 
42.1.3  Applications to Conservation Equations  
With  the  definitions  explained  above,  the  conservation  equations  can  now  be 
written in their discrete form. 
Momentum conservation equation: 
𝑑𝐯𝛼
𝑑𝑡
(𝐱𝑖(𝑡)) =
𝜌𝑖
∂(𝜎 𝛼𝛽)
∂𝑥𝑖
(𝐱𝑖(𝑡)),
where 𝛼, 𝛽 are the space indices. 
The particle approximation of the weak form of this equation is: 
⎜⎛𝜎 𝛼,𝛽(𝐱𝑖)
2 𝐴𝑖𝑗 −
𝜌𝑖
⎝
𝜎 𝛼,𝛽(𝐱𝑗)
𝜌𝑗
(𝐱𝑖) = ∑ 𝑚𝑗
𝑑𝐯𝛼
𝑑𝑡
⎟⎞. 
⎠
𝐴𝑗𝑖
𝑗=1
Energy conservation equation: 
𝑑𝐸
𝑑𝑡
= −
∇𝐯.
(42.16)
(42.17)
(42.18)
The particle approximation of the weak form of this equation is: 
𝑑𝐸
𝑑𝑡
(𝐱𝑖) = −
𝑃𝑖
2 ∑ 𝑚𝑗
𝜌𝑖
𝑗=1
(𝑣(𝐱𝑗) − 𝑣(𝐱𝑖))𝐴𝑖𝑗.
(42.19)
42.1.4  Formulation Available in LS-DYNA  
It  is  easy  from  the  general  formulation  displayed  in  Equation  (42.14)  to  extend 
the SPH formalism to a set of equations of discretization for the momentum equation. 
For example, if we choose the smoothing function to be symmetric, this can lead 
to the following equation: 
𝑑𝐯𝛼
𝑑𝑡
(𝐱𝑖) = ∑ 𝑚𝑗
𝑗=1
⎜⎛𝜎 𝛼,𝛽(𝐱𝑖)
2 +
𝜌𝑖
⎝
𝜎 𝛼,𝛽(𝐱𝑗)
𝜌𝑗
⎟⎞ 𝐴𝑖𝑗. 
⎠
(42.20)
LS-DYNA Theory Manual 
SPH 
This  is  what  we  call  the  “symmetric  formulation”,  which  is  chosen  in  the 
*CONTROL_SPH card (IFORM = 2).  
Another possible choice is to define the momentum equation by: 
⎜⎛𝜎 𝛼,𝛽(𝐱𝑖)
𝜌𝑖𝜌𝑗
⎝
𝜎 𝛼,𝛽(𝐱𝑗)
𝜌𝑖𝜌𝑗
(𝐱𝑖) = ∑ 𝑚𝑗
𝑑𝐯𝛼
𝑑𝑡
⎟⎞. 
⎠
𝐴𝑖𝑗 −
𝐴𝑗𝑖
𝑗=1
(42.21)
This  is  the  “fluid  formulation”  invoked  with  IFORM = 5  which  gives  better 
results than other SPH formulations when fluid material are present, or when material 
with very different stiffness are used. 
42.2  Sorting  
In  the  SPH  method,  the  location  of  neighboring  particles  is  important.    The 
sorting consists of finding which particles interact with which others at a given time.  A 
bucket sort is used that consists of partitioning the domain into boxes where the sort is 
performed.  With this partitioning the closest neighbors will reside in the same box or in 
the  closest  boxes.    This  method  reduces  the  number  of  distance  calculations  and 
therefore the CPU time. 
42.3  Artificial Viscosity 
The artificial viscosity is introduced when a  shock is present.  Shocks introduce 
discontinuities  in  functions.    The  role  of  the  artificial  viscosity  is  to  smooth  the  shock 
over  several  particles.    To  take  into  account the  artificial  viscosity, an  artificial viscous 
pressure term Π𝑖𝑗 [Monaghan & Gingold 1983] is added such that: 
𝑝𝑖 → 𝑝𝑖 + Π𝑖𝑗,
(42.22)
where Π𝑖𝑗 = 1
𝜌̅𝑖𝑗
(−𝛼𝜇𝑖𝑗𝑐 ̅𝑖𝑗 + 𝛽𝜇𝑖𝑗
2 ). 
The notation 𝑋̅̅̅̅̅𝑖𝑗 = 1
the adiabatic sound speed, and 
2 (𝑋𝑖 + 𝑋𝑗) has been used for median between 𝑋𝑖 and 𝑋𝑗, 𝑐 is 
𝑣𝑖𝑗𝑟𝑖𝑗
2 + 𝜂2
𝑟𝑖𝑗
  0
Here, 𝑣𝑖𝑗 = (𝑣𝑖 − 𝑣𝑗), and 𝜂2 = 0.01ℎ̅
𝜇𝑖𝑗 =
{⎧
{⎨
⎩
ℎ̅
𝑖𝑗
if 𝑣𝑖𝑗𝑟𝑖𝑗 < 0
otherwise
(42.23)
2  which prevents the denominator from vanishing. 
𝑖𝑗
SPH 
LS-DYNA Theory Manual 
42.4  Time Integration  
We use a simple and classical first-order scheme for integration.  The time step is 
determined by the expression: 
𝛿𝑡 = 𝐶CFL𝑀𝑖𝑛𝑖 (
ℎ𝑖
𝑐𝑖 + 𝑣𝑖
),
(42.24)
where the factor 𝐶CFL is a numerical constant. 
The calculation cycle is: 
Start
Velocity/positions
LS-DYNA
Accelerations
LS-DYNA
contact, boundary conditions
LS-DYNA
Smoothing length
SPH
Sorting
SPH
Particles forces
SPH
Density, strain rates
SPH
Pressure, thermal energy, stresses
LS-DYNA
42.5  Initial Setup 
Initially,  we  have  a  set  of  particles  with  two  kinds  of  properties:  physical  and 
geometrical properties. 
Physical Properties:
LS-DYNA Theory Manual 
SPH 
The mass, density, constitutive laws are defined in the ELEMENT_SPH and the 
PART cards. 
Geometrical Properties: 
The  geometrical  properties  of  the  model  concern  the  way  particles  are  initially 
placed.  Two different parameters are to be fixed: Δ𝑥𝑖 lengths and the CSLH coefficient. 
These parameters are defined in the SECTION_SPH card. 
A proper SPH mesh must satisfy the following conditions: it must be as regular 
as possible and must not contain too large variations.  
For  instance,  if  we  consider  a  cylinder  SPH  mesh,  we  have  at  least  two 
possibilities: 
The  mesh  number  2  includes  too  many  inter-particle  distance  discrepancies.    
Therefore, the first mesh, more uniform, is better. 
Finite element coupling 
Coupling  finite  elements  and  SPH  elements  is  realized  by  using  contact 
algorithms.  Users can choose any “nodes_to_surface” contact type where the slave part 
is defined with SPH elements and the master part is defined with finite elements.
LS-DYNA Theory Manual 
Element-Free Galerkin 
43    
Element-Free Galerkin 
Mesh-free  methods,  which  construct  the  approximation  entirely  in  terms  of 
nodes,  permit  reduced  restriction  in  the  discretization  of  the  problem  domain  and  are 
less  susceptible  to  distortion  difficulties  than  finite  elements.    For  a  variety  of 
engineering  problems  with  extremely  large  deformation,  moving  boundaries  or 
discontinuities,  mesh-free  methods  are  very attractive.    The  two  most  commonly  used 
approximation  theories  in  mesh-free  methods  are  the  moving  least-squares  (MLS) 
approximation in the Element-free Galerkin (EFG) method [Belytschko et al.  1994], and 
the reproducing kernel (RK) approximation in the reproducing kernel particle method 
(RKPM) [Liu et al.  1995].  Since these two methods lead to an identical approximation 
when monomial basis functions are used, the MLS approximation is used as a basis to 
formulate the mesh-free discrete equations in this section.  
43.1  Moving least-squares 
The Element-free Galerkin method uses the moving least-squares approximation 
to construct the numerical discretization.  The discrete MLS approximation of a function 
𝑢(𝐱), denoted by 𝑢ℎ(𝐱), is constructed by a combination of the monomials as 
𝑢ℎ(𝐱) = ∑ 𝐻𝑖(𝐱)𝑏𝑖(𝐱) ≡ 𝐇T(𝐱)𝐛(𝐱)
,
𝑖=1
(43.1)
where  𝑛  is  the  order  of  completeness  in  this  approximation,  the  monomial  𝐻𝑖(𝐱)  are 
basis functions, and 𝑏𝑖(𝐱) are the coefficients of the approximation. 
The coefficients 𝑏𝑖(𝐱) at any point 𝐱 are depending on the sampling points 𝐱𝐼 that 
are collected by a weighting function 𝑤𝑎(𝐱 − 𝐱𝐼). This weighting function is  defined to 
have a compact support measured by ‘a’, i.e., the sub-domain over which it is nonzero is 
small relative to the rest of the domain.  Each sub-domain ΔΩ𝐼 is associated with a node 
𝐼. The most commonly used sub-domains are disks or balls.  A typical numerical model 
is shown in Figure 43.1.
Element-Free Galerkin 
LS-DYNA Theory Manual 
Figure 43.1.  Graphical representation of mesh-free discretization 
In  this  development,  we  employ  the  cubic  B-spline  kernel  function  as  the 
weighting function: 
− 4 (
)
+ 4 (
‖𝐱 − 𝐱𝐼‖
‖𝐱 − 𝐱𝐼‖
− 4 (
) + 4 (
)
‖𝐱 − 𝐱𝐼‖
‖𝐱 − 𝐱𝐼‖
)
−
(
‖𝐱 − 𝐱𝐼‖
)
𝑤𝑎(𝐱 − 𝐱𝐼) =
⎧2
{
{
{
{
{
⎨
{
{
{
{
{
⎩
for 0 ≤
for 
<
‖𝐱 − 𝐱𝐼‖
‖𝐱 − 𝐱𝐼‖
≤
≤ 1
otherwise
⎫
}
}
}
}
}
⎬
}
}
}
}
}
⎭
(43.2)
The  moving  least-squares  technique  consists  in  minimizing  the  weighted  L2-
Norm   
NP
𝐽 = ∑ Wa(𝐱)
𝐼=1
]
(𝐱 − 𝐱𝐼) [∑ 𝐻𝑖(𝐱)𝑏𝑖(𝐱) − 𝑢(𝐱𝐼)
,
𝑖=1
(43.3)
where  NP  is  the  number  of  nodes  within  the  support  of  𝐱  for  which  the  weighting 
function 𝑤𝑎(𝐱 − 𝐱𝐼) ≠ 0. 
Equation (39.3) can be written in the form 
𝐽 = (𝐇𝐛 − 𝐮)TWa(𝐱)(𝐇𝐛 − 𝐮),
where 
𝐮T = (𝑢1, 𝑢2, ⋯ 𝑢NP),
(43.4)
(43.5)
LS-DYNA Theory Manual 
Element-Free Galerkin 
𝐇 =
{𝐇(𝐱1)}T
⎤
⎡
, 
⋯
⎥
⎢
{𝐇(𝐱NP)}T⎦
⎣
{𝐇(x𝑖)}T = {𝐻1(𝐱𝑖), … 𝐻𝑛(𝐱𝑖)},
𝐖a = diag[𝑤𝑎(𝐱 − 𝐱1), ⋯ , 𝑤𝑎(𝐱 − 𝐱NP)].
To find the coefficients 𝐛 we obtain the extremum of 𝐽 by 
∂𝐽
∂b
= 𝐌[n](𝐱)𝐛(𝐱) − 𝐁(𝐱)𝐮 = 0,
where 𝐌[𝑛](𝐱) is called the moment matrix of 𝑤𝑎(𝐱 − 𝐱𝐼) and is given by 
So we have 
𝐌[n](𝐱) = 𝐇T𝐖a(𝐱)𝐇,
𝐁(𝐱) = 𝐇T𝐖a(𝐱).
𝐛(𝐱) = 𝐌[n]−1
(𝐱)𝐁(𝐱)𝐮.
(43.6)
(43.7)
(43.8)
(43.9)
(43.10)
(43.11)
(43.12)
For 𝐌[𝑛](𝐱) to be invertible, the support of 𝑤𝑎(𝐱 − 𝐱) needs to be greater than a 
minimum  size  that  is  related  to  the  order  of  basis  functions.    Using  the  solution  of 
Equations (43.1), (43.10), (43.11) and (43.12), the EFG approximation is obtained by 
NP
𝑢ℎ(𝐱) = ∑ Ψ𝐼(𝐱)𝑢𝐼
𝐼=1
,
where the EFG shape functions Ψ𝐼(𝐱) are given by 
Ψ𝐼(𝐱) = 𝐇T(𝐱)𝐌[n]−1
(𝐱)𝐁(𝐱),
and 𝚿𝐼(𝐱) are nth-order complete, i.e. 
𝑁𝑃
∑ Ψ𝐼(𝐱)𝑥1𝐼
𝐼=1
𝑞 = 𝑥1
𝑥2𝐼
𝑝𝑥2
𝑞  for  𝑝 + 𝑞 = 0, ⋯ 𝑛.
(43.13)
(43.14)
(43.15)
43.2  Integration constraint and strain smoothing  
The  convergence  of  the  Galerkin  method  for  a  partial  differential  equation  is 
determined  by  approximation  for  the  unknowns  and  the  numerical  integration  of  the 
weak  form.    EFG  shape  functions  with  linear  consistency  can  be  obtained  from  MLS 
approximation  with  linear  basis  functions.    The  employment  of  linearly  consistent 
mesh-free shape functions in the Galerkin approximation, however, does not guarantee
Element-Free Galerkin 
LS-DYNA Theory Manual 
a linear exactness in the solution of the Galerkin method.  It has been shown by Chen et 
al.  [2001] that two integration constraints are required for the linear exactness solution 
in the Galerkin approximation. 
NIT
∑ ∇ΨI(x̂L)AL
𝐿=1
= 0 for  {𝐼: supp(Ψ𝐼) ∩ Γ = 0},
(43.16)
NIT
∑ ∇ΨI(x̂L)AL
𝐿=1
NITh
= ∑ nΨ𝐼(x̃𝐿)𝑠𝐿
𝐿=1
 for  {𝐼: supp(Ψ𝐼) ∩ Γℎ ≠ 0}. 
(43.17)
where Γℎ is the natural boundary, Γ is the total boundary, 𝐧 is the surface normal on Γℎ, 
x̂𝐿  and  𝐴𝐿  are  the  spatial  co-ordinate  and  weight  of  the  domain  integration  point, 
respectively, x̃𝐿 and 𝑠𝐿 are the spatial co-ordinate and weight of the domain of natural 
boundary  integration  point,  respectively,  NIT  is  the  number  of  integration  points  for 
domain integration and NITh is the number of integration points for natural boundary 
integration. 
A strain smoothing method proposed by Chen and Wu [1998] as a regularization 
for  material  instabilities  in  strain  localization  was  extended  in  their  nodal  integration 
method  [Chen  et  al,  2001]  to  meet  the  integration  constraints.    Here,  we  adopt  the 
similar  concept  for  the  domain  integration.    If  starts  with  a  strain  smoothing  at  the 
representative domain of a Gauss point by 
∇̃𝑢𝑖
ℎ(x𝐿) =
𝐴𝐿
∫ ∇𝑢𝑖
Ω𝐿
ℎ(x𝐿)
𝑑Ω, 𝐴𝐿 = ∫ 𝑑Ω
Ω𝐿
,
(43.18)
where  Ω𝐿  is  a  representative  domain  at  each  Guass  point  and  ∇̃  is  the  smoothed 
gradient operator.  By applying divergence theorem to Equation (43.18) to yield 
∇̃𝑢𝑖
ℎ(x𝐿) =
𝐴𝐿
∫ n𝑢𝑖
Γ𝐿
ℎ(x𝐿)
𝑑Γ,
(43.19)
where  Γ𝐿  is  the  boundary  of  the  representative  domain  of  Guass  point  L.  Introducing 
EFG shape functions into Equation (25.22) yields 
∇̃𝑢𝑖
ℎ(x𝐿) = ∑
𝐴𝐿
∫ Ψ𝐼(x)n
Γ𝐿
𝑑Γ ⋅ 𝑑𝑖𝐼 ≡ ∑ ∇̃Ψ𝐼(x𝐿) ⋅ 𝑑𝑖𝐼
. 
(43.20)
It  can  be  shown  that  the  smoothed  EFG  shape  function  gradient  ∇̃Ψ𝐼(xL)  meets  the 
integration  constraints  in  Equations  (43.16)  and  (43.17)  regardless  of  the  numerical 
integration employed.
LS-DYNA Theory Manual 
Element-Free Galerkin 
43.3  Lagrangian strain smoothing for path-dependent 
problems 
To  avoid  the  tensile  instability  caused  by  the  Eulerian  kernel  functions,  the 
Lagrangian kernel functions are implemented in the current LS-DYNA.  
To  introduce  the  Lagrangian  EFG  shape  function  into  the  approximation  of  a 
path-dependent problem, the strain increment Δ𝑢𝑖,𝑗 is computed by 
Δ𝑢𝑖,𝑗 =
∂Δ𝑢𝑖
∂𝑥𝑗
=
∂Δ𝑢𝑖
∂𝑋𝑘
−1.
−1 = Δ𝐹𝑖𝑘𝐹𝑘𝑗
𝐹𝑘𝑗
The strain smoothing of Δ𝑢𝑖,𝑗 at a material pointx𝐿is computed by 
−1(x𝐿),
Δ𝑢̃𝑖,𝑗(x𝐿) = Δ𝐹̃𝑖𝑘(x𝐿)𝐹̃
𝑘𝑗
(43.21)
(43.22)
where 𝐹̃𝑖𝑗(x𝐿) is the Langrangian strain smoothing of deformation gradient and is given 
by 
𝐹̃𝑖𝑗(x𝐿) =
𝐴𝐿
ℎ𝑁𝑗
∫ 𝑢𝑖
Γ𝐿
𝑑Γ + δ𝑖𝑗.
(43.23)
43.4  Galerkin approximation for explicit dynamic 
computation 
The strong form of the initial/boundary value problem for elasto-dynamics is as 
follows: 
ρ𝐮̈ = ∇ ⋅ 𝛔 + 𝐟b in Ω,
(43.24)
with  the  divergence  operator  ∇,  the  body  force  𝐟𝑏,  mass  density  ρ  ,and  with  the 
boundary conditions: 
and initial conditions 
𝐮 = 𝐮0 on Γ𝑢
𝛔 ⋅ 𝐧 = 𝐡 on Γℎ,
𝐮(𝐗, 0) = 𝐮0(𝐗)
𝐮̇(X, 0) = 𝐮̇0(𝐗).
(43.25)
(43.26)
To  introduce  the  Lagrangian  strain  smoothing  formulation  into  the  Galerkin 
approximation, an assumed strain method is employed.  The corresponding weak form 
becomes:
Element-Free Galerkin 
LS-DYNA Theory Manual 
∫ ρδ𝐮 ⋅
Ω𝑥
𝐮̈dΩ + ∫ δ𝛆̃
Ω𝑥
: 𝛔dΩ = ∫ δ𝐮 ⋅
Ω𝑥
𝐟bdΩ + ∫ δ𝐮 ⋅
Γℎ
𝐡dΓ. 
(43.27)
Following the derivation for explicit time integration, the equations to be solved 
have the form 
where 
δ𝐮T𝐌𝐮̈ = δ𝐮T𝐑,
1𝐼,𝑑 ̈
𝐮̈𝐼 = [𝑑 ̈
2𝐼, 𝑑 ̈
𝑀𝐼𝐽 = ∫ ρΨ𝐼(𝐱)Ψ𝐽(𝐱)𝑑Ω =
3𝐼]𝑇 
Ω𝑥
R𝐼 = ∫ 𝐁̃𝐼
Ω𝑥
𝑇(𝐱) ⋅ 𝛔(𝐅̃)𝑑Ω
∫ ρ0Ψ𝐼(𝐗)Ψ𝐽(𝐗)𝑑Ω
Ω𝑋
− [Ψ𝐼(x)𝐡]∣ Γℎ
− ∫ Ψ𝐼(x)𝐟b𝑑Ω
Ω𝑥
(43.28)
(43.29)
, 
where B̃𝐼
coefficient of the approximation or the “generalized” displacement. 
𝑇(x) is the smoothed gradient matrix obtained from Equation (43.22), 𝑑𝑖𝐼 is the 
43.5  Imposition of essential boundary condition 
In  general,  mesh-free  shape  functions  Ψ𝐼  do  not  possess  Kronecker  delta 
properties of the standard FEM shape functions, i.e. 
Ψ𝐼(xJ) ≠ δ𝐼𝐽.
(43.30)
This  is  because,  in  general,  the  mesh-free  shape  functions  are  not  interpolation 
functions.    As  a  result,  a  special  treatment  is  required  to  enforce  essential  boundary 
conditions.  There are many techniques for mesh-free methods to  impose the essential 
boundary condition.  Here, we adopt the transformation method as originally proposed 
for the RKPM method by Chen et al.  [1996]. 
Therefore,  to  impose  the  essential  boundary  conditions  using  kinematically 
admissible  mesh-free  shape  functions  by  the  transformation  method,  Equation  (43.28) 
can be written as  
where 
or 
and 
δ𝐮̂T𝐌̂𝐮̈ = δ𝐮̂T𝐅̂int,
𝐮̂ = 𝐀𝐮; 𝐴𝐼𝐽 = Ψ𝐽(𝑋𝐼).
𝐮 = 𝐀−1𝐮̂,
(43.31)
(43.32)
(43.33)
LS-DYNA Theory Manual 
Element-Free Galerkin 
𝐌̂ = 𝐀−T𝐌𝐀−1; 𝐅̂int = 𝐀−T𝐅int.
(43.34)
A  mixed  transformation  method  [Chen  et  al.    2000]  is  also  considered  as  an 
alternative  to  impose  the  essential  boundary  conditions.    The  mixed  transformation 
method  is  an  improved  transformation  method  that  the  coordinate  transformation  is 
only  applied  for  the  degrees  of  freedom  associated  with  the  essential  and  contact 
boundaries. 
The  nodes  are  partitioned  into  three  groups:  a  boundary  group  𝐺𝐵1  which 
contains all the nodes subjected to kinematic constraints; group 𝐺𝐵2 which contains all 
the  nodes  whose  kernel  supports  cover  nodes  in  group  𝐺𝐵1;  and  internal  group  𝐺𝐼 
which  contains  the  rest  of  nodes.    Nodes  numbers  are  re-arranged  in  the  following 
order in the generalized displacement vector: 
u𝐵1
⎤ 
⎡
u𝐵2
⎥
⎢
u𝐼 ⎦
⎣
where 𝐮𝐵1, 𝐮𝐵2 and 𝐮𝐼 are the generalized displacement vectors associated with groups 
𝐺𝐵1, 𝐺𝐵2 and 𝐺𝐼 respectively.  The transformation in Equation (43.32) is also re-arranged 
as 
𝐮 =
(43.35)
𝐮̂ = [𝐮̂𝐵
𝐮̂𝐼 ] [ΛBB ΛBI
ΛIB ΛII ] [𝐮𝐵
𝐮𝐼 ] ≡ 𝚲̂𝐮,
where 
𝐮̂B = [û𝐵1
û𝐵2
] ; 𝐮B = [u𝐵1
u𝐵2
= [Λ𝐼𝐵1 Λ𝐼𝐵2].
] ; 𝚲BB = [ΛB1B1 ΛB1B2
ΛB2𝐵1 ΛB2B2
] ; 𝚲BI = [
Λ𝐵2𝐼] ; 𝚲IB
Here, we introduce a mixed displacement vector 𝐮∗, 
𝐮∗ = [𝐮̂𝐵
𝐮𝐼 ] [ΛBB ΛBI
] [𝐮𝐵
𝐮𝐼 ] ≡ 𝚲∗𝐮,
and Λ∗ and its inverse are: 
𝚲∗ = [ΛBB ΛBI
] ; 𝚲∗−1
= [ΛBB−1
−ΛBB−1
ΛBI
].
Only the inversion of Λ𝐵𝐵is required in Equation (22.68.15). 
(43.36)
(43.37)
(43.38)
(43.39)
Using  the  mixed  coordinates  in  Equation  (43.38),  the  transformed  discrete 
Equation (43.31) becomes   
δ𝐮∗T𝐌∗𝐮̈∗ = δ𝐮∗T𝐑∗,
(43.40)
where
Element-Free Galerkin 
LS-DYNA Theory Manual 
𝐌∗ = 𝐀∗−T𝐌𝐀∗−1; 𝐑∗ = 𝐀∗−T𝐑.
(43.41)
The  computation  in  Equations  (43.41)  is  much  less  intensive  than  that  in 
Equation  (43.31),  especially  when  the  number  of  boundary  and  contact  nodes  is  much 
smaller than the number of interior nodes. 
43.6  Mesh-free Shell 
The extension of explicit mesh-free solid analysis to shell analysis is described in 
this  section.  Two  projection  methods  are  developed  to  generate  the  shell  mid-surface 
using  the  moving-least-squares  approximations.    A  co-rotational,  updated  Lagrangian 
procedure  is  adopted  to  handle  arbitrarily  large  rotations  with  moderate  strain 
responses of the shell  structures.  A local boundary integration method in conjunction 
with  the  selective  reduced  integration  method  is  introduced  to  enforce  the  linear 
exactness and relieve shear locking. 
43.6.1  Mesh-free Shell Surface Representation 
Surface  reconstruction  from  disorganized  nodes  is  very  challenging  in  three 
dimensions.  The problem is ill posed, i.e., there is no unique solution.  Lancaster et al.  
[1981] first proposed a fast surface reconstruction using  moving least squares  method.  
Their  approach  was  then  applied  to  the  computational  mechanics  under  the  name 
‘mesh-free  method’.    Implicitly,  the  mesh-free  method  uses  a  combination  of  smooth 
basis functions (primitives) to find a scalar function such that all data nodes are close to 
an  iso-contour  of  that  scalar  function  in  a  global  sense.    In  reality,  the  shell  surface 
construction  using  the  3D  mesh-free  method  is  inadequate.    This  is  because  the 
topology of the real surface can be very complicated in three dimensions.  Without the 
information on the ordering or connectivity of nodes, the reconstructed surface will not 
be able to represent shell intersections, exterior boundaries and shape corners. 
In  our  development  of  mesh-free  shells,  we  assume  that  a  shell  surface  is 
described  by  a  finite  element  mesh.    This  can  be  easily  accomplished  by  converting  a 
part  of  shell  finite  elements  into  mesh-free  zone.    With  the  connectivity  of  nodes 
provided  by  the  finite  element  mesh,  a  shell  surface  can  be  reconstructed  with  mesh-
free interpolation from the nodal positions 
𝐱̅ = Ψ̃𝐼(𝐗)𝐱𝐼,
(43.42)
where 𝐱𝐼 is the position vector of the finite element node on the shell surface and Ψ̃𝐼(𝐗) 
is  the  mesh-free  shape  function.    In  the  above  surface  representation,  a  3D  arbitrary 
shell surface needs to be projected to a 2D plane.  Two approaches for the projection of 
mesh-free shell surface are used:
LS-DYNA Theory Manual 
Element-Free Galerkin 
Projection
Figure 43.2.  Mesh-free shell global approach 
•  Global  parametric  representation:  The  whole  shell  surface  is  projected  to  a 
parametric  plane  and  the  global  parametric  coordinates  are  obtained  with  a 
parameterization algorithm from the patch of finite elements. 
•  Local  projection  representation:  A  local  area  of  the  shell  is  projected  to  a  plane 
based on the existing element where the evaluated point is located. 
Global parametric approach 
In  the  global  approach,  a  mesh-free  zone  with  a  patch  of  finite  elements  is 
mapped  onto  a  parametric  plane  with  an  angle-based  triangular  flattening  algorithm 
[Sheffer and de Sturler 2001], . The idea of this algorithm is to compute 
a projection that minimizes the distortion of the FE mesh angles.  The mesh-free shape 
functions are defined in this parametric domain and given by 
Ψ̃𝐼(𝐗) = Ψ̃𝐼(𝜉 , 𝜂),
(43.43)
where (𝜉 , 𝜂) is the parametric coordinates corresponding to a point X. 
Local projection approach 
Different  from  the  parameterization  algorithm  that  constructs  the  surface 
globally,  we  reconstruct  the  surface  locally  by  projecting  the  surrounding  nodes  onto 
one element.  In the local projection method, nodes in elements neighboring the element 
where  the  evaluated  point  is  located  (for  example,  the  element  i  in  Figure  43.3)  are 
projected  onto  the  plane  which  the  element  defines  (the  “M-plane”  in  Figure  43.3).  In 
this figure, (𝑥̂, 𝑦̂, 𝑧̂)𝑖 is a local system defined for each projected plane and (𝑥̅, 𝑦̅, 𝑧̅)𝐼 is a 
nodal  coordinate  system  defined  for  each  node  where 𝑧̅  is  the  initial  averaged  normal 
direction.  
The  mesh-free  shape  functions  are  then  defined  with  those  locally  projected 
coordinates of the nodes 
Ψ𝐼(𝐗) = Ψ𝐼(𝑥̂, 𝑦̂).
(43.44)
Element-Free Galerkin 
LS-DYNA Theory Manual 
zI¯
M-plane
yI¯
xI¯
^
zi
^
yi
M-plane
^
xi
Figure 43.3.  Mesh-free shell local projection 
However, the shape functions obtained directly above are non-conforming, i.e. 
Ψ𝐼(𝐗𝐽)∣
M−plane
≠ Ψ𝐼(𝐗𝐽)∣
N−plane
.
(43.45)
When  the  shell  structure  degenerates  to  a  plate,  the  constant  stress  condition 
cannot  be  recovered.    To  remedy  this  problem,  an  area-weighed  smoothing  across 
different  projected  planes  is  used  to  obtain  the  conforming  shape  functions  that  are 
given by 
Ψ̃𝐼(𝐗) = Ψ̃𝐼(𝑥̂, 𝑦̂) =
NIE
𝑖=1
∑ Ψ𝐼(𝑥̂𝑖, 𝑦̂𝑖)𝐴𝑖
𝑁𝐼𝐸
∑ 𝐴𝑖
𝑖=1
. 
(43.46)
where NIE is the number of surrounding projected planes that can be evaluated at point 
X,  𝑨𝒊  is  the  area  of  the  element  𝑖,  and  (𝑥̂𝑖, 𝑦̂𝑖)  is  the  local  coordinates  of  point  X  in  the 
projected plane 𝑖.  
With this smoothing technique, we can prove that the modified shape functions satisfy 
at  least  the  partition  of  unity  property  in  the  general  shell  problems.    This  property  is 
important for the shell formulation to preserve the rigid-body translation. 
When the shell degenerates to a plate, we can also prove that the shape functions 
obtained  from  this  smoothing  technique  will  meet  the  n-th  order  completeness 
condition as 
NP
∑ Ψ̃𝐼(𝐗)𝑋1𝐼
𝐼=1
𝑖 𝑋2𝐼
𝑗 𝑋3𝐼
= 𝑋1
𝑖 𝑋2
𝑗 𝑋3
𝑘,
𝑖 + 𝑗 + 𝑘 = 𝑛.
(43.47)
This is a necessary condition for the plate to pass the constant bending patch test. 
43.6.2  Updated Lagrangian Formulation and Co-rotational Procedure 
The  mesh-free  shell  formulation  is  based  on  the  Mindlin-Reissner  plate  theory, 
thus the geometry and kinematical fields of the shell can be described with the reference
LS-DYNA Theory Manual 
Element-Free Galerkin 
z^
ζV3
y^
x^
x¯
Figure 43.4.  Geometry of a shell. 
surface  and  fiber  direction.    The  modified  Mindlin-Reissner  assumption  requires  that 
the motion and displacement of the shell are linear in the fiber direction.  Assume that 
the  reference  surface  is  the  mid-surface  of  the  shell,  the  global  coordinates  and 
displacements at an arbitrary point within the shell body are given by 
𝐱 = 𝐱̅ + ζ
𝐕3,
(43.48)
where  𝐱̅  and  𝐮̅̅̅̅  are  the  position  vector  and  displacement  of  the  reference  surface, 
respectively. 𝐕3 is the fiber director and 𝐔 is the displacement resulting from the fiber 
rotation . ℎ is the length of the fiber. 
𝐮 = 𝐮̅̅̅̅ + ζ
(43.49)
𝐔.
With the mesh-free approximation, the motion and displacements are given by 
𝐱(𝜉 , 𝜂, 𝜁 ) = 𝐱̅(𝜉 , 𝜂) + 𝐕(𝜉 , 𝜂, 𝜁 ) ≈ ∑ Ψ̃𝐼(𝜉 , 𝜂)𝐱𝐼
𝑁𝑃
𝑁𝑃
+ ∑ Ψ̃𝐼(𝜉 , 𝜂)
𝐼=1
𝐼=1
𝜁 ℎ𝐼
𝐕3𝐼,
(43.50)
Initial configuration
V3
X¯
u¯
V3
x¯
Deformed Configuration
Figure 43.5.  Deformation of a shell.
Element-Free Galerkin 
LS-DYNA Theory Manual 
𝐮(𝜉 , 𝜂, 𝜁 ) = 𝐮̅̅̅̅(𝜉 , 𝜂) + 𝐔(𝜉 , 𝜂, 𝜁 ) ≈ ∑ Ψ̃𝐼(𝜉 , 𝜂)𝐮𝐼
𝑁𝑃
𝑁𝑃
+ ∑ Ψ̃𝐼(𝜉 , 𝜂)
𝐼=1
𝐼=1
𝜁 ℎ𝐼
[−𝐕2𝐼 𝐕1𝐼] {
𝛼𝐼
𝛽𝐼
}
,(43.51)
where  𝐱𝐼  and  𝐮𝐼  are  the  global  coordinates  and  displacements  at  mesh-free  node  𝐼, 
respectively. 𝐕3𝐼 is the unit vector of the fiber director and 𝐕1𝐼, 𝐕2𝐼 are the base vectors 
of  the  nodal  coordinate  system  at  node  𝐼.  𝛼𝐼  and  𝛽𝐼  are  the  rotations  of  the  director 
vector  𝐕3𝐼  about  the  𝐕1𝐼  and  𝐕2𝐼  axes.  ℎ𝐼  is  the  thickness.    The  variables  with  a 
superscripted bar refer to the shell mid-surface. Ψ̃𝐼 is the 2D mesh-free shape functions 
constructed based on one of the two mesh-free surface representations described in the 
previous  section,  with  (𝜉 , 𝜂)  either  the  parametric  coordinates  or  local  coordinates  of 
the evaluated point. 
The  local  co-rotational  coordinate  system  (𝑥̂, 𝑦̂, 𝑧̂)  is  defined  at  each  integration 
point on the shell reference surface, with 𝑥̂ and 𝑦̂ tangent to the reference surface and 𝑧̂ 
in the thickness direction . The base vectors are given as 
𝐞̂1 =
𝐱,ξ
∥𝐱,ξ∥
, 𝐞̂3 =
𝐱,ξ × 𝐱,η
∥𝐱,ξ × 𝐱,η∥
, 𝐞̂2 = 𝐞̂3 × 𝐞̂1.
(43.52)
In  order  to  describe  the  fiber  rotations  of  a  mesh-free  node  in  a  shell,  we 
introduce  a  nodal  coordinate  system  whose  three  base  vectors  are  𝐕1,  𝐕2  and  𝐕3,  see 
Figure 43.6, where 𝐕3 is the fiber director at the node and 𝐕1, 𝐕2 are defined as follows 
𝐕1 =
𝐱̂ × 𝐕3
∣𝐱̂ × 𝐕3∣
, 𝐕2 = 𝐕3 × 𝐕1.
(43.53)
The rotation of the fiber director is then obtained from the global rotations:  
𝛽} = [
{
𝐕1
T] Δθ,
𝐕2
Δθ = [Δ𝜃1 Δ𝜃2 Δ𝜃3]T.
(43.54)
LS-DYNA Theory Manual 
Element-Free Galerkin 
V3
V2
z^
y^
zs^
ys^
xs^
x^
V1
Figure 43.6.  Local co-rotational and nodal coordinate systems. 
In  the  local  co-rotational  coordinate  system,  the  motion  and  displacements  are 
approximated by the mesh-free shape functions 
NP
x̂i = ∑ Ψ̃Ix̂iI
I=1
NP
+ ζ ∑ Ψ̃I
I=1
hI
𝑉̂3𝑖𝐼
,
NP
ûi = ∑ Ψ̃IûiI
I=1
NP
+ ζ ∑ Ψ̃I
I=1
hI
[−V̂2iI V̂1iI] {
αI
βI
.
}
The Lagrangian smoothed strains [Chen et al.  2001b] are given by 
ε̃m = ∑ 𝐁̃I
m𝐝̂
, ε̃b = ζ ∑ 𝐁̃I
b𝐝̂
, ε̃s = ∑ 𝐁̃I
s𝐝̂
,
(43.55)
(43.56)
(43.57)
where  the  smoothed  strain  operators  are  calculated  by  averaging  the  consistent  strain 
operators over an area around the evaluated point 
m(𝐱𝑙) =
𝐁̃𝐼
𝐴𝑙
m𝑑𝐴
∫ 𝐁̂𝐼
Ω𝑙
, 𝐁̃𝐼
b(𝐱𝑙) =
𝐴𝑙
b𝑑𝐴
∫ 𝐁̂𝐼
Ω𝑙
, 𝐁̃𝐼
s(𝐱𝐿) =
𝐴𝐿
∫ 𝐁̂𝐼
Ω𝐿
s𝑑𝐴
, 
(43.58)
with 
𝐁̂𝐼
=
⎡Ψ̃𝐼,𝑥
⎢
⎢
⎢
⎢
⎢
⎢
⎣
0 −𝐽13
−1Ψ̃𝐼
Ψ̃𝐼,𝑦
0 −𝐽23
−1Ψ̃𝐼
Ψ̃𝐼,𝑦 Ψ̃𝐼,𝑥
0 −𝐽23
−1Ψ̃𝐼
ℎ𝐼
ℎ𝐼
ℎ𝐼
𝑉̂2𝑥𝐼
𝑉̂2𝑦𝐼
−1Ψ̃𝐼
𝐽13
−1Ψ̃𝐼
𝐽23
𝑉̂2𝑥𝐼 − 𝐽13
−1Ψ̃𝐼
ℎ𝐼
𝑉̂2𝑦𝐼
−1Ψ̃𝐼
𝐽23
ℎ𝐼
ℎ𝐼
ℎ𝐼
𝑉̂1𝑥𝐼
𝑉̂1𝑦𝐼
𝑉̂1𝑥𝐼 + 𝐽13
−1Ψ̃𝐼
⎤
⎥
⎥
⎥
⎥
⎥
⎥
𝑉̂1𝑦𝐼⎦
ℎ𝐼
,  (43.59)
Element-Free Galerkin 
LS-DYNA Theory Manual 
xl
xL
Figure 43.7.  Integration scheme for mesh-free shells. 
𝐁̂𝐼
b =
⎡0
⎢
⎢
⎢
⎢
⎢
⎢
⎣
0 −Ψ̃𝐼,𝑥
0 −Ψ̃𝐼,𝑦
0 −Ψ̃𝐼,𝑦
ℎ𝐼
ℎ𝐼
ℎ𝐼
𝑉̂2𝑥𝐼
𝑉̂2𝑦𝐼
Ψ̃𝐼,𝑥
Ψ̃𝐼,𝑦
𝑉̂2𝑥𝐼 − Ψ̃𝐼,𝑥
ℎ𝐼
𝑉̂2𝑦𝐼 Ψ̃𝐼,𝑦
ℎ𝐼
ℎ𝐼
ℎ𝐼
𝑉̂1𝑥𝐼
𝑉̂1𝑦𝐼
𝑉̂1𝑥𝐼 + Ψ̃𝐼,𝑥
⎤
⎥
⎥
⎥
, 
⎥
⎥
⎥
𝑉̂1𝑦𝐼⎦
ℎ𝐼
(43.60)
𝐁̂𝐼
s =
−1Ψ̃𝐼
⎡0
⎢⎢⎢
⎣
𝑉̂2𝑦𝐼 − 𝐽23
0 Ψ̃𝐼,𝑦 −𝐽33
ℎ𝐼
ℎ𝐼
and 𝐉−1 is the inverse of the Jacobian matrix at the integration point.  The local degrees-
of-freedom are 
⎤
⎥⎥⎥
,  (43.61)
𝑉̂1𝑧𝐼⎦
0 Ψ̃𝐼,𝑥 −𝐽33
𝑉̂1𝑦𝐼 + 𝐽23
𝑉̂1𝑥𝐼 + 𝐽13
𝑉̂2𝑥𝐼 − 𝐽13
ℎ𝐼
ℎ𝐼
ℎ𝐼
ℎ𝐼
ℎ𝐼
ℎ𝐼
−1Ψ̃𝐼
𝐽33
−1Ψ̃𝐼
𝐽33
−1Ψ̃𝐼
−1Ψ̃𝐼
−1Ψ̃𝐼
−1Ψ̃𝐼
−1Ψ̃𝐼
𝑉̂2𝑧𝐼
𝑉̂1𝑧𝐼
𝑉̂2𝑧𝐼
The internal nodal force vector is 
𝐝̂
𝐼 = [𝑢̂𝑥𝐼 𝑢̂𝑦𝐼 𝑢̂𝑧𝐼 𝛼𝐼 𝛽𝐼]T.
int = ∫ 𝐁̃I
𝐅̂I
mT
σ̂
dΩ + ∫ ζ𝐁̃I
bT
σ̂
sT
dΩ + ∫ 𝐁̃I
σ̂
dΩ.
(43.62)
(43.63)
The  above  integrals  are  calculated  with  the  local  boundary  integration  method.  
Each background finite element is divided into four integration zones, shown as  Ω𝑙 in 
Figure 43.7. In order to avoid shear locking in the analysis of thin shells, the shear term 
(third term in Eq. (43.63)), should be under-integrated by using one integration zone in 
each background element (Ω𝐿 in Figure 43.7). Accordingly, the co-rotational coordinate 
systems are defined separately at the center of each integration zone, as shown in Figure 
43.6. 
The  use  of  the  updated  Lagrangian  formulation  implies  that  the  reference 
coordinate system is defined by the co-rotational system in the configuration at time t.
LS-DYNA Theory Manual 
Element-Free Galerkin 
Therefore,  the  local  nodal  force  and  displacement  vectors  referred  to  this  coordinate 
system must be transformed to the global coordinate system prior to assemblage.
LS-DYNA Theory Manual 
Linear shells 
44    
Linear shells 
44.1  Shells for Linear Analysis 
It is common to construct elements for linear analysis by the superimposition of a 
plate and a membrane element.  If the base plates and membrane elements involve only 
three translational degrees-of-freedom and two in-plane rotational degrees-of-freedom, 
the  resulting  element  then  contains  5  degrees-of-freedom  per  node  since  there  is  an 
unconstrained rotational degree-of-freedom normal to the mid surface of the shell.  This 
unconstrained mode can cause problems when linking the shell to other elements such 
as beam elements in three-dimensional space.  For this reason, the linear elements in LS-
DYNA are based on published formulations  that include a drilling degree-of-freedom, 
which  is  added  to  the  membrane  part  of  the  element  to  form  a  24  degree-of-freedom 
shell element.  These elements pass all patch tests, have 6 rigid body modes, and have 
no spurious mechanisms. 
44.2  Wilson’s Shell (element #20) 
This quadrilateral element is constructed as described above and is discussed in 
more detail by Wilson [2000].  The triangular element, which is an 18 degree-of-freedom 
complement  to  the  quadrilateral  elements,  follows  the  same  procedure.    In  a  linear 
analysis in LS-DYNA, automatic sorting is invoked if a mesh has both quadrilateral and 
triangular elements within a single part ID.  This sorting ensures the proper treatment 
of triangles.   
44.2.1  Plate Element 
The  4  node  quadrilateral  plate  element  is  based  on  the  8  node,  quadratic 
quadrilateral  plate  element,  which  has  16  rotational  degrees-of-freedom,  i.e.,  two  per
Linear shells 
LS-DYNA Theory Manual 
Plate
Membrane
Figure 44.1.  Shell as assembly of plate and membrane elements 
nodal point.  The implementation in LS-DYNA directly follows the textbook by Wilson 
[2000] where the complete details of the element are provided.  A condensed overview 
is given here.  The shell theory makes the following assumptions: 
•The fiber remains straight and inextensible 
•The normal stress in the thickness direction is zero 
The local x and y rotations of the shell are interpolated from the equations: 
𝜃𝑥(𝑟, 𝑠) = ∑ 𝑁𝑖
(𝑟, 𝑠)𝜃𝑥𝑖 + ∑ 𝑁𝑖
(𝑟, 𝑠)Δ𝜃𝑥𝑖
𝑖=1
𝑖=5
𝜃𝑦(𝑟, 𝑠) = ∑ 𝑁𝑖
(𝑟, 𝑠)𝜃𝑦𝑖 + ∑ 𝑁𝑖
(𝑟, 𝑠)Δ𝜃𝑦𝑖,
𝑖=1
𝑖=5
(44.1)
where  nodes  5-8  are  at  the  mid  side  of  the  element.    The  interpolation  functions  are 
given by 
𝑁1 =
𝑁2 =
𝑁3 =
𝑁4 =
(1 − 𝑟)(1 − 𝑠) 𝑁5 =
(1 + 𝑟)(1 − 𝑠)   𝑁6 =
(1 + 𝑟)(1 + 𝑠)   𝑁7 =
(1 − 𝑟)(1 + 𝑠) 𝑁8 =
(1 − 𝑟2)(1 − 𝑠)
(1 + 𝑟)(1 − 𝑠2) 
(1 − 𝑟2)(1 + 𝑠) 
(1 − 𝑟)(1 − 𝑠2).
(44.2)
In his formulation, Wilson resolves the rotation of the mid side node into tangential and 
normal components relative to the shell edges.  The tangential component is set to zero 
leaving the normal component as the unknown, which reduces the rotational degrees-
of-freedom from 16 to 12, see Figure 44.2. 
Δ𝜃𝑥 = sin𝛼𝑖𝑗Δ𝜃𝑖𝑗
Δ𝜃𝑦 = −cos𝛼𝑖𝑗Δ𝜃𝑖𝑗
(44.3)
LS-DYNA Theory Manual 
Linear shells 
ΔΘ
ΔΘ
ΔΘ
ij
ij
i = 1, 2, 3, 4
j = 2, 3, 4, 1
m =5, 6, 7, 8
Figure 44.2.  Element edge [Wilson, 2000] 
𝜃𝑥(𝑟, 𝑠) = ∑ 𝑁𝑖
(𝑟, 𝑠)𝜃𝑥𝑖 + ∑ 𝑀𝑥𝑖
(𝑟, 𝑠)Δ𝜃𝑖
𝑖=1
𝑖=5
𝜃𝑦(𝑟, 𝑠) = ∑ 𝑁𝑖
(𝑟, 𝑠)𝜃𝑦𝑖 + ∑ 𝑀𝑦𝑖
(𝑟, 𝑠)Δ𝜃𝑖.
𝑖=1
𝑖=5
(44.4)
Ultimately,  the  4  mid  side  rotations  are  eliminated  by  using  static  condensation,  a 
procedure that makes this shell very costly if used in explicit calculations. 
The local 𝑥 and 𝑦 displacements relative to the mid surface are functions of the 𝑧-
coordinate and rotations: 
𝑢𝑥(𝑟, 𝑠) = 𝑧𝜃𝑦(𝑟, 𝑠)
𝑢𝑦(𝑟, 𝑠) = −𝑧𝜃𝑥(𝑟, 𝑠).
(44.5)
Wilson shows, where it is assumed that the normal displacement along each side 
is cubic, that the transverse shear strain along each side is given by, 
𝛾𝑖𝑗 =
(𝑢𝑧𝑗 − 𝑢𝑧𝑖) −
(𝜃𝑖 + 𝜃𝑗) −
Δ𝜃𝑖𝑗,
which can be rewritten, referring to Figure 44.3 as: 
𝛾𝑖𝑗 =
(𝑢𝑧𝑗 − 𝑢𝑧𝑖) −
sin𝛼𝑖𝑗
(𝜃𝑥𝑖 + 𝜃𝑥𝑗) +
cos𝛼𝑖𝑗
(𝜃𝑦𝑖 + 𝜃𝑦𝑗) −
Δ𝜃𝑖𝑗, 
The nodal shears are then written in terms of the side shears as 
sin𝛼𝑖𝑗
sin𝛼𝑘𝑖
which can be inverted to obtain the nodal shears: 
cos𝛼𝑖𝑗
cos𝛼𝑘𝑖
𝛾𝑖𝑗
𝛾𝑘𝑖
] = [
[
] [
𝛾𝑥𝑧
𝛾𝑦𝑧
],
(44.6)
(44.7)
(44.8)
Linear shells 
LS-DYNA Theory Manual 
ki
ΔΘ
ki
ki
ij
ΔΘ
ij
ij
i = 1, 2, 3, 4
j = 2, 3, 4, 1
m =5, 6, 7, 8
xz
yz
Figure 44.3.  Nodal and edge shear strains [Wilson 2000]. 
𝛾𝑥𝑧
𝛾𝑦𝑧
[
] =
cos𝛼𝑖𝑗sin𝛼𝑘𝑖 − cos𝛼𝑘𝑖sin𝛼𝑖𝑗
[
sin𝛼𝑘𝑖
−sin𝛼𝑖𝑗
−cos𝛼𝑘𝑖
cos𝛼𝑖𝑗
] [
𝛾𝑖𝑗
𝛾𝑘𝑖
]. 
(44.9)
The  standard  bilinear  basis  functions  are  used  to  interpolate  the  nodal  shears  to  the 
integration points. 
44.2.2  Membrane Element 
The  membrane  element,  which  is  also  coded  from  Wilson’s  textbook  [2000],  is 
based on the eight node isoparametric element, see Figure 44.4.  
The  inplane  displacement  field  for  the  8  node  membrane  is  interpolated,  using 
the serendipity shape functions with the mid-side relative displacements, from: 
𝑢𝑥(𝑟, 𝑠) = ∑ 𝑁𝑖
(𝑟, 𝑠)𝑢𝑥𝑖 + ∑ 𝑁𝑖
(𝑟, 𝑠)Δ𝑢𝑥𝑖
𝑖=1
𝑖=5
𝑢𝑦(𝑟, 𝑠) = ∑ 𝑁𝑖
(𝑟, 𝑠)𝑢𝑦𝑖 + ∑ 𝑁𝑖
(𝑟, 𝑠)Δ𝑢𝑦𝑖.
𝑖=1
𝑖=5
(44.10)
It is desired to replace the mid side relative displacment by drilling rotations at 
the  corner  nodes.    Consider  Figure  44.5:  the  mid-side  normal  displacements  along  the 
edge are parabolic, i.e.,  
Δ𝑢𝑖𝑗 =
𝐿𝑖𝑗
(Δ𝜃𝑗 − Δ𝜃𝑖),
(44.11)
LS-DYNA Theory Manual 
Linear shells 
while the mid-side tangential displacements are interpolated linearly from the end node 
displacements, thus, 
Δ𝑢𝑥(𝑟, 𝑠) = cos𝛼𝑖𝑗Δ𝑢𝑖𝑗 = cos𝛼𝑖𝑗
𝐿𝑖𝑗
Δ𝑢𝑦(𝑟, 𝑠) = −sin𝛼𝑖𝑗Δ𝑢𝑖𝑗 = −sin𝛼𝑖𝑗
(Δ𝜃𝑗 − Δ𝜃𝑖)
𝐿𝑖𝑗
(Δ𝜃𝑗 − Δ𝜃𝑖),
𝑢𝑥(𝑟, 𝑠) = ∑ 𝑁𝑖
(𝑟, 𝑠)𝑢𝑥𝑖 + ∑ 𝑀𝑥𝑖
(𝑟, 𝑠)Δ𝜃𝑖
𝑖=1
𝑖=5
𝑢𝑦(𝑟, 𝑠) = ∑ 𝑁𝑖
(𝑟, 𝑠)𝑢𝑦𝑖 + ∑ 𝑀𝑦𝑖
(𝑟, 𝑠)Δ𝜃𝑖.
𝑖=1
𝑖=5
(44.12)
(44.13)
This element has one singularity in the drilling mode of equal corner rotations, see 
Figure 44.6. 
Ibrahimbegovic and Wilson [1991] added a penalty formulation to the potential 
energy of the element to eliminate the singularity.  The following penalty term connects 
the averaged nodal rotation to the continuum mechanics rotation 
(
∂𝑢𝑥
∂𝑦
−
∂𝑢𝑦
∂𝑥
) − 𝜔
(44.14)
Figure 44.4.  Eight node membrane element.
Linear shells 
LS-DYNA Theory Manual 
Δuy
ΔΘ
Δux
i = 1, 2, 3, 4
j = 2, 3, 4, 1
m = 5, 6, 7, 8
Δuij
ij
Lij
ΔΘ
Figure  44.5.    Corner  node  drilling  rotations  and  mid  side  edge  normal
displacement [Wilson, 2000]. 
Figure 44.6.  Zero energy mode 
at  the  center  of  the  element.    The  element  performance  is  highly  insensitive  to  the 
chosen  value  of  the  penalty  factor  and  some  fraction  of  the  elastic  modulii,  G  or  E,  is 
frequently used.  
•  5, 8 or 9 point quadrature can be applied.    The 5 and 8 point schemes induce a 
‘soft’ first deformational mode, whereas the 9 point Gaussian quadrature results 
in a stiffer mode. 
•  A  membrane  locking  correction  (Taylor)  is  applied  to  (i)  alleviate  a  membrane-
bending interaction associated with the drilling degrees of freedom and (ii) allow
LS-DYNA Theory Manual 
Linear shells 
the standard application of the consistent nodal load at the edge.  The correction 
has a slight stiffening effect . 
•  A warping correction is applied using the rigid link correction . 
44.3  Assumed Strain/Membrane with Drilling Degree-of-
freedom (element #18) 
44.3.1  Membrane Element 
Formulation is the same as above for element type 20. 
44.3.2  Plate Element 
The  Discrete  Kirchhoff  Quadrilateral  element  is  an  excellent  thin  shell  element 
based on 
•  Rotational field is interpolated using the 8-node isoparametric parent element. 
•  Transverse  displacement  w  assumed  as  cubic  along  the  sides  and  collocated 
along  the  sides  and  at  the  nodes  using  the  Kirchhoff  condition  that  equates  the 
fiber  rotation  to  the  slope.    The  Kirchhoff  assumptions  are  satisfied  along  the 
entire boundary of the element. 
•  The rotational field about an axis parallel to the side is constrained linearly along 
the sides. 
The warping correction is applied as above. 
Flat Element
Figure 44.7.  Flat element
Linear shells 
LS-DYNA Theory Manual 
44.4  Differences between Element Types 18 and 20. 
The DKQ does not account for transverse shear because it locally enforces the 
Kirchhoff condition.  Hence, element type 20 is better for layered composites and 
thick plates.
LS-DYNA Theory Manual 
Random Geometrical Imperfections 
45    
Random Geometrical Imperfections 
45.1  Introduction to Random Geometrical Imperfections 
Using Karhunen-Loève Expansions 
through  using  Karhunen-Loève  expansions 
There  are  different  methods  of  incorporating  imperfections,  depending  on  the 
availability  of  accurate  imperfection  data.    The  method  implemented  into  LS-DYNA 
v971  uses  a  spectral  decomposition  of  geometrical  or  thickness  uncertainty,  more 
.    To  specify  the  covariance  of  the  random  field  of  the  geometrical 
imperfections  or  thickness  variation,  two  methods  are  available.    The  first  is  to  use 
available  experimentally-measured  imperfection  fields  as  input  for  a  principal 
component analysis based on pattern (face) recognition literature.  This method reduces 
the cost of the resulting eigen-analysis.  The second is to specify the covariance function 
analytically  and  to  solve  the  resulting  Friedholm  integral  equation  of  the  second  kind 
using  a  wavelet-Galerkin  approach,  also  obtained  from  literature.    Six  different 
analytical  covariance  kernels  (e.g.,  exponential  and  triangular)  are  available  for 
selection.  
45.2  Methodology 
45.2.1  Generation of random fields using Karhunen-Loève expansion  
The  Karhunen-Loève  expansion  (e.g.,  Ghanem  and  Spanos  [2003])  provides  an 
attractive  way  of  representing  a  random  (stochastic)  field  (process)  through  a  spectral 
decomposition, ϖ, as a function of x (e.g., two spatial variables): 
∞
𝜛(x, 𝜃) = 𝜛̅(x) + ∑ √𝜆i𝜉𝑖(𝜃)𝑓𝑖(x)
, 
𝑖=1
(45.1)
where  the  𝜉𝑖  are  uncorrelated  zero-mean  random  variables  with  unit  variance,  and 
𝜛̅(x)is  the  average  random  field  or  mean  of  the  process.    The  functions  𝑓𝑖  are  the
Random Geometrical Imperfections 
LS-DYNA Theory Manual 
eigenfunctions of the covariance kernel, C, with 𝜆𝑖 the associated eigenvalues, obtained 
from the spectral decomposition of the covariance function via the solution on a domain 
𝐷 of the Fredholm integral equation of the second kind, 
∫ 𝐶(x1, x2)𝑓𝑖(x1)𝑑x1
= 𝜆𝑖𝑓𝑖(x2).
The eigenfunctions form an orthogonal set 
∫ 𝑓𝑖(x)𝑓𝑗(x)𝑑x
= 𝛿𝑖𝑗.
Normally, a finite 𝑀 number of terms are kept in the series expansion: 
𝜛(x, 𝜃) = 𝜛̅(x) + ∑ √𝜆i𝜉𝑖(𝜃)𝑓𝑖(x)
.
(45.2)
(45.3)
(45.4)
𝑖=1
If 𝜛 is Gaussian, then 𝜉𝑖 are also Gaussian.  For non-Gaussian processes (with arbitrary 
but specified marginal distributions), 𝜉𝑖 are unknown.  Phoon et al ([2002a], [2005]) give 
an iterative procedure for obtaining 𝜉𝑖 given a target marginal distribution. 
45.2.2  Solution of Fredholm integral of the second kind for analytical covariance 
functions  
The  Wavelet-Galerkin  method  (Phoon  et  al  [2002])  is  used  to  perform  the 
solution, and can be described as follows. 
By  defining  a  set  of  basis  functions:  𝜑1(𝑥),  𝜑2(𝑥),…,𝜑𝑁(𝑥),  each  eigenfunction 
𝑓𝑖(𝑥) can be approximated by the linear combination: 
𝑓𝑖(𝑥) = ∑ 𝑑𝑖𝑘
𝜑𝑘(𝑥),
𝑘=1
(45.5)
where  the  𝑑𝑖𝑘  are  constant  coefficients.    By  substituting  (45.5)  into  Fredholm  equation 
(45.2) (using a scalar 𝑥 (one-dimensional random process) as an example) and writing as 
an error: 
∫ 𝐶(x1, x2) ∑ 𝑑𝑖𝑘𝜑𝑘(𝑥1)𝑑x1
𝑘=1
− 𝜆𝑖 ∑ 𝑑𝑖𝑘𝜑𝑘(𝑥1)
= 0.
𝑘=1
(45.6)
By making the error orthogonal to the basis functions: 
⎢⎡∫ 𝐶(x1, x2) ∑ 𝑑𝑖𝑘𝜑𝑘(𝑥1)𝑑x1
⎣
𝑘=1
⎥⎤
− 𝜆𝑖 ∑ 𝑑𝑖𝑘𝜑𝑘(𝑥1)
⎦
𝑘=1
𝜑𝑗(𝑥2)𝑑𝑥2 = 0, 
(45.7)
∫
we get 
∑ 𝑑𝑖𝑘
𝑘=1
⎢⎡∬ 𝐶(x1, x2)
⎣
𝜑𝑘(𝑥1)𝜑𝑗(𝑥2)𝑑x1𝑑x2
⎥⎤ − 𝜆𝑖 ∑ 𝑑𝑖𝑘
⎦
𝑘=1
⎢⎡∫ 𝜑𝑘(𝑥2)𝜑𝑗(𝑥2)𝑑x2
⎣
⎥⎤
⎦
= 0,
(45.8)
LS-DYNA Theory Manual 
Random Geometrical Imperfections 
or the eigensystem 
𝐀𝐃 = 𝚲𝐁𝐃
with  Λ𝑖𝑗 = 𝛿𝑖𝑗𝜆𝑗.    Orthogonal  wavelets  𝜓(𝑥)  are  used  (∫ 𝜓𝑗(x)𝜓𝑘(x)𝑑x
functions, 
𝐟𝑖(𝑥) = ∑ 𝑑𝑖𝑘
𝑘=1
𝜓𝑘(𝑥) = 𝛙T(𝑥)𝐃(𝑖),
so that the covariance function can be expressed as: 
(45.9)
= ℎ𝑗𝛿𝑗𝑘)  as  basis 
(45.10)
𝐶(𝐱1, 𝐱2) = ∑ ∑ 𝐴̅𝑗𝑘𝜓𝑗(𝐱1)𝜓𝑘(𝐱2) = 𝛙T(𝐱1)𝐀̅̅̅̅̅̅
𝛙(𝐱2),
(45.11)
𝑗=1
where 𝐀̅̅̅̅̅̅ is the 2D wavelet transform of 𝐶(𝐱1, 𝐱2) given by 
𝑘=1
𝐴̅𝑗𝑘 =
ℎ𝑗ℎ𝑘
∫ ∫ 𝐶(𝐱1, 𝐱2)𝜓𝑗(𝐱1)𝜓𝑘(𝑥2)𝑑x1𝑑x2
.
Substituting (45.10) and (45.11) into (45.2), we again get an eigenvalue problem 
𝛙T(𝑥)𝐀̅̅̅̅̅̅𝐇𝐃(𝑖) = 𝜆𝑖𝛙T(𝑥)𝐃(𝑖).
(45.12)
(45.13)
2⁄ 𝐃(𝑖)  and  𝐀̂ =
Or,  equating  coefficients  of  𝛙T  and  using  the  transformation  𝐃̂ (𝑖) = 𝐇
2⁄ , the eigensystem 
2⁄ 𝐀̅̅̅̅̅̅𝐇
The  eigenvectors  from (45.14)  are  transformed  to  the  eigen  functions  (of (45.9))  by  the 
equation: 
𝐀̂𝐃̂ (𝑖) = 𝜆𝑖𝐃̂ (𝑖).
(45.14)
𝐟𝑖(𝑥) = 𝛙T(𝑥)𝐇−1
2⁄ 𝐃̂ (𝑖).
(45.15)
The  double  integral  in  (45.12)  is  constructed  using  two  successive  1D  discrete 
wavelet  transforms  in  the  form  of  Mallat’s  tree  algorithm  (Phoon  et  al  [2002a]).    Haar 
wavelets  are  used  because  of  their  simplicity  and  ability  to  capture  the  field 
characteristics.  The eigenfunctions (45.15) and associated eigenvalues 𝜆𝑖 can be used to 
construct  random  fields  (using  (45.4))  with  the  same  second-order  statistics  as  the 
covariance model used.  
The available covariance functions (Ghanem and Spanos [2003]), are: 
•  Exponential covariance function (First-order Markov process (autoregressive)),  
𝐶(x1, x2) = exp (
−|𝑥1 − 𝑥2|
𝐿𝑐
)
(45.16)
•  Triangular covariance function
Random Geometrical Imperfections 
LS-DYNA Theory Manual 
𝐶(x1, x2) = 1 −
|𝑥1 − 𝑥2|
𝐿𝑐
•  Sine covariance function 
𝐶(x1, x2) =
sin𝐿𝑐(𝑥1 − 𝑥2)
𝐿𝑐(𝑥1 − 𝑥2)
•  Squared exponential covariance function 
𝐶(x1, x2) = exp (
−|𝑥1 − 𝑥2|2
𝐿𝑐
)
•  Wiener-Levy covariance function 
𝐶(x1, x2) = min(x1, x2)
•  Uniformly modulated nonstationary covariance function 
𝐶(x1, x2) = exp(−(𝑥1 − 𝑥2))exp
−|𝑥1 − 𝑥2|
𝐿𝑐
with 𝐿𝑐 the correlation length in the respective direction. 
(45.17)
(45.18)
(45.19)
(45.20)
(45.21)
45.2.3  Generating eigenfunctions from experimentally measured fields  
If experimentally measured random fields are available, then the eigenfunctions 
and eigenvalues in (45.1) or (45.4) can be determined from the second-order statistics of 
the  measurements.    Following  the  pattern  recognition  method  proposed  by  Turk  and 
Pentland [1991], the procedure described next is used.  
Given  a  set  of  𝑀  field  measurements,  e.g.,  geometrical  imperfections  on  an 
𝑁1 × 𝑁2  mesh,  we  can  represent  the  measurements  as  1-D  vectors  of  length  𝑁1 × 𝑁2, 
i.e., Γ1, …, Γ𝑀.  The average vector is defined by 
𝚿 =
∑ 𝚪𝑛
𝑛=1
,
(45.22)
allowing  us  to  define the  deviation  of  each measured  field  from  the  average,  also  as  a 
vector:  𝚽𝑖 = 𝚪𝑖 − 𝚿.    Combining  the  deviation  vectors  into  a  covariance  matrix,  𝐂,  we 
get 
𝐂 =
∑ 𝚽𝑛𝚽𝑛
𝑛=1
= 𝐀𝐀T,
(45.23)
where  𝐀 = [𝚽1  𝚽2 … 𝚽𝑀]. 
  The  covariance  matrix  has  a  set  of  orthonormal 
eigenvectors, 𝐟𝑖, and associated eigenvalues, 𝜆𝑖 obtained through a principal component 
analysis, i.e.,
LS-DYNA Theory Manual 
Random Geometrical Imperfections 
The eigenpairs are chosen such that 
𝐀𝐀T𝐟𝑖 = 𝜆𝑖𝐟𝑖.
is a maximum, subject to 
𝜆𝑖 =
∑(𝐟𝑖
𝑛=1
T𝚽𝑛)
,
T𝐟𝑘 = 𝛿𝑙𝑘,
𝐟𝑖
(45.24)
(45.25)
(45.26)
with  𝛿  the  Kronecker  delta.    As  the  size  of  the  covariance  matrix  is  (𝑁1 × 𝑁2)2, 
determining  the  eigenvectors and  eigenvalues  in  (41.24)  can  be  a  time-consuming  and 
memory-intensive  task  for  large  measurement  meshes.    This  computation  can  be 
simplified  if  the  number  of  measurement  samples  is  less  than  the  mesh  count  (𝑀 <
𝑁1 × 𝑁2),  as  there  are  then  only  𝑀– 1,  rather  than  𝑁1 × 𝑁2,  meaningful  eigenvectors.  
This is done by considering the eigenvectors of another matrix 𝐋 = 𝐀T𝐀, as embodied 
in the eigensystem 
𝐀T𝐀v𝑖 = 𝜇𝑖𝐯𝑖.
Premultiplying both sides in (20.1.6) by 𝐀, we get 
𝐀𝐀T𝐀𝐯𝑖 = 𝜇𝑖𝐀𝐯𝑖,
(45.27)
(45.28)
which implies that the 𝑀 –  1 eigenvectors, 𝐀𝐯𝑖, are also eigenvectors of 𝐀𝐀Tor 𝐂.  The 
𝑇 𝚽𝑛.  
eigensystem in (20.1.6), however, is only size (𝑀 × 𝑀), as 𝐋 = 𝐀T𝐀, where 𝐿𝑛𝑚 = 𝚽𝑚
Once  the  eigenvectors  of 𝐋  are  obtained,  the required  eigenfunctions, 𝐟𝑖,  are  recovered 
through the linear combination 
𝐟𝑖 = ∑ v𝑖𝑘𝚽𝑘
𝑘=1
,
𝑖 = 1, … , 𝑀
(45.29)
The 𝑀 –  1 eigenvalues of 𝐋 and 𝐂 are identical, i.e., 𝜆𝑖 = 𝜇𝑖.  Finally 𝐟𝑖and 𝜆𝑖 are used in 
(45.4) to construct the required Karhunen-Loève expansion of the random fields.
LS-DYNA Theory Manual 
Frequency Domain 
46    
Frequency Domain 
46.1  Frequency Response Functions 
Frequency  response  function  (FRF)  is  a  characteristic  of  a  system  that  has  a 
measured or computed response resulting from a known applied input.  Mathematical-
ly it is a transfer function and expresses the structural response to an applied force as a 
function of frequency.  The response can be given in terms of displacement, velocity, or 
acceleration.    Frequency  response  functions  are  complex  functions,  with  real  and 
imaginary  components.    They  can  also  be  written  in  terms  of  magnitude  and  phase 
pairs. 
46.1.1  FRF Computations 
FRF  is  computed  using  mode  superposition  method,  in  frequency  domain.  
When damping is included, the dynamic response of a system is governed by 
𝐦𝐮̈ + 𝐜𝐮̇ + 𝐤𝐮 = 𝐩(𝑡),
(46.1.1)
where  𝐦,  𝐜  and  𝐤  are  the  mass,  damping  and  stiffness  matrices,  𝐩(𝑡)  is  the  external 
force. 
Using  the  mode  superposition  method,  the  displacement  response  can  be 
expressed by 
𝐮 = ∑ 𝜙𝑛𝑞𝑛(𝑡)
= Φq,
(46.1.2)
𝑛=1
where 𝜙𝑛 is the n-th mode shape and 𝑞𝑛(𝑡) is the n-th modal coordinates. 
With  the  substitution  of  Equation  (46.1.2)  into  Equation  (46.1.1),  the  governing 
equation can be rewritten as 
Pre-multiplying by ΦT gives 
𝐦𝚽𝐪̈ + 𝐜𝚽𝐪̇ + 𝐤𝚽𝐪 = 𝐩(𝑡).
𝐌𝐪̈ + 𝐂𝐪̇ + 𝐊𝐪 = 𝐩(𝑡),
(46.1.3)
(46.1.4)
Frequency Domain 
LS-DYNA Theory Manual 
The  orthogonality  of  natural  modes  implies  that  the  following  square  matrices  are 
diagonal: 
where the diagonal elements are  
𝐌 ≡ 𝚽𝐓𝐦𝚽,
𝐊 ≡ 𝚽𝐓𝐤𝚽,
𝐌𝒏 = 𝛟𝒏
𝐓𝐦𝛟𝒏,
𝐊𝒏 = 𝛟𝒏
𝐓𝐤𝛟𝒏
(46.1.5)
(46.1.6)
Since  𝐦  and  𝐤  are  positive  definite,  the  diagonal  elements  of  𝐌  and  𝐊  are  positive.  
They are related by 
The square matrix 𝐂 is obtained similarly as follows 
𝐊𝒏 = 𝛚𝒏
𝟐𝐌𝒏.
𝐂 = 𝚽𝐓𝐜𝚽.
(46.1.7)
(46.1.8)
𝐂 may or may not be diagonal, depending on the distribution of damping in the 
system.  If 𝐂 is diagonal (the diagonal elements are 𝐶𝑛 = 𝜙𝑛
represents N uncoupled differential equations in modal coordinates 𝑞𝑛, and the system 
is said to have classical damping and the systems possess the same natural modes as 
those of the undamped system.  Only the classical damping is considered in this 
approach. 
𝑇𝑐𝜙𝑛), Equation (46.1.4) 
The right hand side vector (generalized force) 𝐏(𝑡) is 
For  an  N-DOF  system  with  classical  damping,  each  of  the  N  differential 
equations in modal coordinates is 
𝐏(𝑡) = ΦT𝑝(𝑡)
(46.1.9)
or,  
𝑀𝑛𝑞 ̈𝑛 + 𝐶𝑛𝑞 ̇𝑛 + 𝐾𝑛𝑞𝑛 = 𝑃𝑛(𝑡)
where the modal damping coefficient 
𝑞 ̈𝑛 + 2𝜁𝑛𝜔𝑛𝑞 ̇𝑛 + 𝜔𝑛
2𝑞𝑛 =
𝑃𝑛(𝑡)
𝑀𝑛
ζ  is defined as 
𝜁𝑛 =
𝐶𝑛
2𝑀𝑛𝜔𝑛
(46.1.10)
(46.1.11)
(46.1.12)
Applying Fourier transform to both sides of Equation (46.1.11), one obtains 
(−𝜔2 + 2𝑖𝜁𝑛𝜔𝑛𝜔 + 𝜔𝑛
2)𝑞𝑛(𝜔) =
𝑃𝑛(𝜔)
𝑀𝑛
(46.1.13)
The structural displacement response in frequency domain can be represented as  
𝐮(𝜔) = ∑
𝑛=1
𝜙𝑛
2)
(−𝜔2 + 2𝑖𝜁𝑛𝜔𝑛𝜔 + 𝜔𝑛
𝑃𝑛(𝜔)
𝑀𝑛
46-2 (Frequency Domain)
LS-DYNA Theory Manual 
Frequency Domain 
Thus  the  displacement  frequency  response  function  (Compliance)  can  be 
expressed  as  (suppose  that  the  excitation  is  applied  at  node  j  and  the  response  is 
evaluated for node k) 
𝐅𝐑𝐅𝒖(𝑥𝑗, 𝑥𝑘, 𝜔) = ∑
𝑛=1
𝜙𝑛(𝑥𝑘)
2)
(−𝜔2 + 2𝑖𝜁𝑛𝜔𝑛𝜔 + 𝜔𝑛
𝑃̃𝑛(𝑥𝑗)
𝑀𝑛
The velocity frequency response function (Mobility) can be expressed as 
𝐅𝐑𝐅𝒗(𝑥𝑗, 𝑥𝑘, 𝜔) = 𝜔𝑖 ∑
𝑛=1
𝜙𝑛(𝑥𝑘)
2)
(−𝜔2 + 2𝑖𝜁𝑛𝜔𝑛𝜔 + 𝜔𝑛
𝑃̃𝑛(𝑥𝑗)
𝑀𝑛
(46.1.15)
(46.1.16)
The acceleration frequency response function (Accelerance) can be expressed as 
𝐅𝐑𝐅𝒂(𝑥𝑗, 𝑥𝑘, 𝜔) = −𝜔2 ∑
𝑛=1
𝜙𝑛(𝑥𝑘)
2)
(−𝜔2 + 2𝑖𝜁𝑛𝜔𝑛𝜔 + 𝜔𝑛
𝑃̃𝑛(𝑥𝑗)
𝑀𝑛
where 
~
n xP
(
)
is obtained as 
𝑃̃𝑛(𝑥𝑗) = 𝜙𝑛
𝑇𝑝̃(𝑥𝑗)
(46.1.17)
(46.1.18)
and 
(~
jxp
force excitation, 
)
is the space distribution of the harmonic force excitation (in the case of point 
(~
jxp
=
1)
 at node j in specified direction of excitation and 0 elsewhere). 
46.1.2  About the damping 
Damping can be given in several forms .  
A  very  common  type  of  damping  used  in  the  nonlinear  analysis  of  structure  is  to 
assume that the damping matrix is proportional to the mass and stiffness matrices, or 
This  type  of  damping  is  normally  referred  to  as  Rayleigh  damping.    For 
𝐜 = 𝛼𝐦 + 𝛽𝐤
(46.1.19)
classically damped system,  
Due to the orthogonality of the mass and stiffness matrices, it can be rewritten as 
2𝝎𝒏𝜁𝑛 = 𝜙𝑛
𝑇𝐜𝜙𝑛
(46.1.20)
or, 
2𝝎𝒏𝜁𝑛 = 𝛼 + 𝛽𝜔𝑛
𝜁𝑛 =
2𝜔𝑛
+
𝜔𝑛
(46.1.21)
(46.1.22)
Frequency Domain 
LS-DYNA Theory Manual 
46.2   ACOUSTIC FEM 
A  frequency  domain  acoustic  finite  element  method  has  been  implemented  in 
LS-DYNA,  to  model  the  acoustic  behavior  of  a  confined  acoustic  fluid  volume.    This 
method is based on nodal velocity/pressure formulation.  Three types of elements are 
available.  They are hexahedron, pentahedron, and tetrahedron elements. 
46.2.1  Theory basis 
The governing equation for the acoustic problem is the Helmholtz equation. 
∇𝟐𝑝 + 𝑘𝟐𝑝 = 0
(46.2.1)
where  𝑝  is  the  acoustic  pressure;  𝑘 = 𝜔/𝑐  is  called  the  wave  number;  𝜔 = 2𝜋𝑓   is  the 
circular frequency of the acoustic wave; and 𝑐 is the wave speed. 
For vibro-acoustic problems, the boundary condition is given as follows, 
𝜕𝑝
𝜕𝑛
= −𝑖𝜌𝜔𝑣𝑛 
(46.2.2)
where 𝑛 is the normal vector pointing outside from the acoustic volume; 𝑖 = √−1 is the 
imaginary unit; 𝜌 is the acoustic fluid density and 𝑣𝑛 is the normal velocity. 
Using  the  weighted  residue  technique  and  taking  the  shape  function  𝑁𝑖  as  the 
weighting function, the governing equation can be written as 
∫ ∇2𝑝𝑁𝑖𝑑𝑉
+ ∫ 𝑘2𝑝𝑁𝑖𝑑𝑉
= 0 
Using the Green’s theorem, Equation (2.3) can be written as 
− ∫ ∇𝑝∇𝑁𝑖𝑑𝑉
+ 𝑘2 ∫ 𝑝𝑁𝑖𝑑𝑉
= − ∫
𝜕𝑝
𝜕𝑛
𝑁𝑖𝑑Γ
(46.2.3)
(46.2.4)
With  the  substitution  of  the  boundary  condition  (46.2.2)  into  Equation  (46.2.4), 
and taking the nodal pressure as the unknown variables, a linear equation system can 
be established and solved in frequency domain.  Since there is only one variable on each 
node, this method is very fast.
LS-DYNA Theory Manual 
Rotor Dynamics 
47    
 Rotor Dynamics 
47.1  Introduction 
Rotor  dynamics is  a  specialized  branch  of engineering  science concerned  with  the 
behavior and diagnosis of rotating structures.  It is a study of vibration of rotating parts 
found in a wide range of equipment including engine, turbine, aircraft, hard disk drive 
and  more.    The  analysis  of  the  rotator  dynamics  involves  two  coordinate  systems: 
rotating and fixed coordinate systems.  The equations of motion in the two coordinate 
systems are both introduced. 
47.2  Two Coordinate systems 
The  interpretation  of  rotational  phenomena  requires  the  introduction  of  a  rotating 
coordinate  system  in  relation  to  the  fixed  coordinate  system.    Figure  1.1  depicts  the 
relationship between the two coordinate systems. OXYZ is the fixed coordinate system 
and oxyz is the rotating coordinate system. R is the location vector of the disk center; r 
is the location vector of a point P with respect to the rotating coordinate system. Let the 
velocity of rotation be defined as (cid:3).
Rotor Dynamics 
LS-DYNA Theory Manual 
Figure 1.1 A rotating disk in two coordinate systems. 
The position of the point P with respect to OXYZ is 𝒓 ̅, so 
𝒓 ̅ = 𝑹 + 𝒓.
The velocity of point P is: 
𝒗̅̅̅̅ =
𝑑𝒓 ̅
𝑑𝑡
=
𝑑𝑹
𝑑𝑡
+
𝑑𝒓
𝑑𝑡
= 𝑽 + 𝒗 + 𝜴 × 𝒓,
(47.1)
(47.2)
where 𝑽  (=𝑑𝑹
coordinate system. 
𝑑𝑡 ) is the velocity of the origin o; 𝒗 is the velocity of point P in the rotating 
The acceleration of point P can be calculated as:  
𝒂̅ =
𝑑𝒗̅̅̅̅
𝑑𝑡
=
𝑑𝑽
𝑑𝑡
+
𝑑𝒗
𝑑𝑡
+
𝑑(𝜴 × 𝒓 )
𝑑𝑡
= 𝑨 + 𝒂 + 𝟐𝜴 × 𝒗 + 𝜴 × (𝜴 × 𝒓) +
𝒅𝜴
𝑑𝑡
× 𝒓, 
(47.1)
where, 𝑨 is the acceleration of the origin o,  𝒂 is the acceleration of point P in rotating 
coordinate system. 
We assume that the origin of the rotating coordinate system is fixed, so that: 
By substituting (1.4) to (1.3): 
𝑽 = 𝑨 = 𝟎 .
𝒂̅ = 𝒂 + 𝟐𝜴 × 𝒗 + 𝜴 × (𝜴 × 𝒓) +
𝑑𝜴
𝑑𝑡
× 𝒓 .
(47.2)
(47.3)
47.3  Forces in the Rotating Coordinate System 
We now place a particle with mass m into the position of the point P we were following.  
From (1.5), we can express the force of the particle in the rotating system as:
LS-DYNA Theory Manual 
Rotor Dynamics 
𝑭 = 𝑚𝒂 = 𝑚𝒂̅ − 2𝑚𝜴 × 𝒗 − 𝑚𝜴 × (𝜴 × 𝒓) − 𝑚
𝐝𝛀
𝐝t
× 𝐫. 
(47.4)
The  first  term  𝑚𝒂̅  is  the  force  in  the  fixed  coordinate  system.    All  other  terms  on  the 
right hand side are inertia forces arising in the rotating system.  The Coriolis force is the 
following quantity: 
The third term produces the familiar centrifugal force: 
𝑭𝑪 = −2𝑚𝜴 × 𝒗.
𝑭𝑪𝒇 = −𝑚𝜴 × (𝜴 × 𝒓).
(47.5)
(47.6)
The  last  term  introduces  the  Euler  fore  when  there  is  a  nonzero  rate  of  change  in  the 
magnitude of the rotation vector: 
𝑭𝑬 = −𝑚
𝒅𝜴
𝒅𝑡
× 𝒓.
(47.7)
47.4  Transformation between Coordinate Systems 
Let’s  assume  that  the  rotation  axis  coincides  with  one  of  the  axis  of  the  rotating 
coordinate system, specifically to the z axis.  An arbitrary rotation axis will be discussed 
later.  In this case, the rotational velocity becomes:  
𝜴 = 0 ∙ 𝒊 + 0 ∙ 𝒋 + Ω ∙ 𝒌.
(47.8)
We  further  restrict  our  computations  to  constant  rotational  velocity;  hence  the  Euler 
force will not appear in the formulations (Euler force is easy to add to our equations if 
the rotational velocity is not constant though).  
We write the location of a particle in the rotating coordinate system as: 
𝒓 = {
}.
It is transformed to the location in the fixed system as follows: 
𝐫 ̅ =
{⎧𝑥̅
}⎫
𝑦̅
𝑧̅⎭}⎬
⎩{⎨
=
𝑐𝑜𝑠Ωt −𝑠𝑖𝑛Ωt
⎢⎡
𝑐𝑜𝑠Ωt
𝑠𝑖𝑛Ωt
⎣
⎥⎤ {
1⎦
} = 𝑯 {
}.
(47.9)
(47.10)
𝑯  is  the  transformation matrix.   It  is  easy  to get  that   𝑯 𝑇𝑯 = 𝑰,  where 𝑰  is  he  identity 
matrix. Other matrices that may be used later are also given here: 
𝑯̇ = Ω
−𝑠𝑖𝑛Ωt −𝑐𝑜𝑠Ωt
⎢⎡
𝑐𝑜𝑠Ωt −𝑠𝑖𝑛Ωt
⎣
⎥⎤ = Ω𝐇̅̅̅̅̅̅,
0⎦
(47.11)
Rotor Dynamics 
LS-DYNA Theory Manual 
𝑯̈ = Ω2
sinΩt
−𝑐𝑜𝑠Ωt
⎢⎡
−𝑠𝑖𝑛Ωt −𝑐𝑜𝑠Ωt
⎣
⎥⎤ = Ω2𝐇̿̿̿̿̿̿,
0⎦
𝑯̅̅̅̅̅ 𝑇𝑯 =
−1
⎢⎡
⎣
⎥⎤ = 𝑷,
0⎦
𝑯 𝑇𝑯̅̅̅̅̅   =
0 −1
⎢⎡
⎣
⎥⎤ = 𝐏T = −𝑷,
0⎦
𝑯̅̅̅̅̅ 𝑇𝑯̅̅̅̅̅ 𝑇 =
⎢⎡
⎣
⎥⎤ = 𝐉.
0⎦
(47.12)
(47.13)
(47.14)
(47.15)
47.5  Equation of Motion in Rotating Coordinate System 
When  the  particle  undergoes  a  nodal  translation  in  the  rotating  coordinate  system  as 
shown in Figure 1.2, it can be defined as: 
𝒖 = {
}.
The location vector in the fixed coordinate is: 
𝒓 ̅ = 𝑯(𝒓 + 𝒖)
(47.16)
(47.17)
After calculate the velocity in the fixed coordinate system, we can get the kinetic energy 
due to translation displacement as: 
𝑇 =
𝑚Ω2
(𝒓𝑇𝑱𝒓 + 2𝒓𝑇𝑱𝒖 + 𝒖𝑇𝑱𝒖) +
(2Ω𝒖̇𝑇𝑷𝑇𝒓 + 2Ω𝒖𝑇𝑷𝒖̇ + 𝒖̇𝑇𝒖̇). 
(47.18)
Figure 1.2 Translation nodal displacement.
LS-DYNA Theory Manual 
Rotor Dynamics 
Figure 1.3 Rotational nodal displacement. 
The nodal displacement of the point can also be rotational as shown in Figure 1.3. We 
assume small rotation of the rotating point: 
{⎧𝜑
}⎫
𝜃⎭}⎬
⎩{⎨
The  nodal  rotation  requires  the  consideration  of  mass  and  inertia.    The  center  of  the 
mass  point  is  coincident  with  the  node.    The  inertia  moment  can  be  given  with  the 
concentrated mass input of commercial finite element codes, or they can be defined in 
connection  with  the  surrounding  mass  point,  or  even  with  a  simplified  model  by 
attaching six submasses to the node, as shown in figure 1.4. 
𝛉 =
(47.19)
.
Figure 1.4 Node with six masses located at offset x’, y’ and z’ from the node center. 
With  this,  the  location  vector  in  the  fixed  coordinate  is  of  the  form  if  only  considers 
rotational displacement:  
where 
𝒓 ̅ = 𝑯(𝒓 + 𝒖) = 𝑯(𝒓 + 𝑨𝛉),
𝑨 =
−𝑧′
𝑦′ −𝑥′
𝑧′ −𝑦′
⎤. 
𝑥′
⎥
0 ⎦
⎡
⎢
⎣
(47.20)
(47.21)
Then we can get the kinetic energy due to rotational displacement as: 
𝑇 =
𝑚Ω2
(𝒓𝑇𝑱𝒓 + 𝟐𝒓𝑇𝑱𝑨𝛉 + 𝛉𝑻 𝑨𝑇𝑱𝑨𝛉) +
(2Ω𝒓𝑇𝑷𝑨𝛉̇ + 2Ω𝛉𝑇𝑨𝑇𝑷𝑨𝛉̇ + 𝛉̇𝑇𝑨𝑇𝑨𝛉̇). (47.22)
Rotor Dynamics 
LS-DYNA Theory Manual 
Applying  Lagrange’s  equation,  then  we  can  obtain  the  final  equation  of  motion  as 
follows: 
𝑪𝒖
𝟎 𝑪𝛉
] {𝒖̇
𝑴𝒖
𝟎 𝑴𝛉
] {𝒖̈
[
𝛉̈} + 2Ω [
𝛉̇} − Ω2 [
where  𝑴𝒖  and  𝑴𝛉  are  the  mass  and  inertia  matrices;  𝑪𝒖  and  𝑪𝛉  are  the  gyroscopic 
matrices; 𝒁𝒖  and  𝒁𝛉  are  the  centrifugal  softening  matrices;  𝑭𝒄𝒖  and  𝑭𝒄𝛉  are  centrifugal 
force.  Note that we don’t consider the other system damping and external force terms 
here, but they can be added to (1.25) accordingly. 
} = {
(47.23)
] {
}, 
𝒁𝒖
𝟎 𝒁𝛉
𝑭𝒄𝒖
𝑭𝒄𝛉
47.6  Equation of Motion in Fixed Coordinate System 
The location vector in the fixed coordinate is:  
𝒓 ̅ = 𝑯(𝒓 + 𝒖) = 𝑯𝒓 + 𝒖̅.
(47.24)
Here the 𝒖̅  represents the displacement of the point in the fixed coordinate system due 
to the nodal translation displacement.  Similar analysis as in section 1.5 can be done for 
the  equation  of  motion  in  fixed  coordinate  system.    We  only  give  the  final  equation 
here: 
[
] {𝒖̇
] {𝒖̅
𝛉̅̅̅̅̈} + Ω [
𝑴𝒖̅
𝟎 𝑴𝛉̅̅̅̅̅
0 𝑪𝛉̅̅̅̅̅
where 𝑴𝒖̅ and 𝑴𝛉̅̅̅̅̅ are the mass and inertia matrices; 𝑪𝛉̅̅̅̅̅ is the gyroscopic matrix; 𝑭𝒄𝒖̅ is 
the centrifugal force. All of them are written in the fixed coordinate system. Note that 
only  nodal  rotations  contributed  to  the  gyroscopic  matrix.    Same  as  before,  we  don’t 
consider  the  other  system  damping  and  external  force  terms  here,  but  they  can  be 
added to (1.27) accordingly. 
𝛉̇} = {
𝑭𝒄𝒖̅
(47.25)
},
47.7  Arbitrary Rotation Axis 
All the above analysis is based on the assumption that the rotation axis is coincide with 
the  z-axis.    Here  we  will  give  a  way  to  transform  all  variables  back  to  global  if  the 
rotation  axis  is  not  coincide  with  the  z-axis  (Figure  1.5).    The  transformation  matrix 
from z axis to rotation axis is denoted as T and it is easy to get  𝑻 𝑇𝑻 = 𝑰 . 
47-6 (Rotor Dynamics)
LS-DYNA Theory Manual 
Rotor Dynamics 
Figure 1.5 Rotation axis not coincide with z axis. 
The location vector in the fixed coordinate becomes:  
𝒓 ̅ = 𝑻 𝑇𝑯(𝒓′ + 𝒖′).
(47.26)
where  𝒓′  and  𝒖′    are  the  location  vector  and  displacement  in  the  coordinate  system 
Ox’y’z’, in which the z axis is transformed to the rotation axis z’ by rotation matrix 𝑻.At 
the same time: 
𝒓′ = 𝑻𝒓 ,
𝒖′ = 𝑻𝒖.
(47.27)
(47.28)
where,  𝒓 and 𝒖   are  the  location  vector  and  displacement    in  the  rotating  coordinate 
system Oxyz. 
The equation of motion in (1.25) and (1.27) can be simplified written as:  
And the force term can be written as  
𝑴𝟎𝒂 + 𝑪𝟎𝒗 + 𝑲𝟎𝒖 = 𝑭𝟎,
𝑭𝟎 = 𝒇𝟎𝒓,
(47.29)
(47.30)
By substituting (1.28), (1.29) and (1.30) to the equation of motion, we can get new mass, 
damping, stiffness matrices and force vector as follows: 
𝑴 = 𝑻 𝑻 𝑴𝟎𝑻 ,
𝑪 = 𝑻 𝑻 𝑪𝟎𝑻,
𝑲 = 𝑻 𝑻 𝑲𝟎𝑻,
𝑭 = 𝑻 𝑻 𝒇𝟎𝑻𝒓.
(47.31)
(47.32)
(47.33)
(47.34)
So the equation of motion becomes:
Rotor Dynamics 
LS-DYNA Theory Manual 
𝑴𝒂 + 𝑪𝒗 + 𝑲𝒖 = 𝑭 .
(47.35)
After the equation of motion is obtained, it can then be solved using the implicit solver.  
Especially, the damping and stiffness matrices are related to the rotational velocity, so 
the eigen-frequencies might change with the change of rotational velocity.  A diagram 
to  represent  this  relationship  is  called  Campbell  diagram.    An  example  is  given  in 
Figure 1.6.
LS-DYNA Theory Manual 
Rotor Dynamics 
Figure 1.6 A disk is spinning with the center axis, the mode frequencies change with the 
increase of rotating speed.
LS-DYNA Theory Manual 
References 
48    
References 
Abbo A.J., S.W. Sloan, “A Smooth Hyperbolic Approximation to the Mohr-Coulomb 
Yield Criterion,” Computers and Structures, Vol 54, No 1, 1995. 
Addessio, F.L., D.E. Carroll, J.K. Dukowicz, F.H. Harlow, J.N. Johnson, B.A. Kashiwa, 
M.E. Maltrud, H.M. Ruppel, “CAVEAT:  A Computer Code for Fluid Dynamics 
Problems with Large Distortion and Internal Slip,” Report LA-10613-MS, UC-32, Los 
Alamos National Laboratory (1986). 
Ahmad, S., Irons, B.M. and Zienkiewicz, O.C., “Analysis of Thick and Thin Shell 
Structures by Curved Finite Elements,” Int.  J. Numer.  Meths.  Eng., 2 (1970). 
Amsden, A. A., and Hirt, C. W., “YAQUI: An Arbitrary Lagrangian-Eulerian Computer 
Program for Fluid Flow at All Speeds,” Los Alamos Scientific Laboratory, LA-5100 
(1973). 
Amdsden, A., A., Ruppel, H. M., and Hirt, C. W., “SALE: A Simplified ALE Computer 
Program for Fluid Flow at All Speeds,” Los Alamos Scientific Laboratory (1980). 
Argyris, J.H., Kelsey, S., and Kamel, H., “Matrix Methods of Structural Analysis: A 
Precis of recent Developments,” Matrix Methods of Structural Analysis, Pergamon 
Press (1964). 
Arruda, E., and M. Boyce, "A Three-Dimensional Constitutive Model for the Large 
Stretch Behavior of Rubber Elastic Materials," published in the Journal of the Mechanics 
and Physics of Solids, Vol. 41, No.  2, 389-412 (1993). 
Auricchio, F., Taylor, R.L. and Lubliner J., “Shape-memory alloys: macromodelling and 
numerical simulations of the superelastic behavior”, Computer Methods in Applied 
Mechanics and Engineering 146, 281-312 (1997).
References 
LS-DYNA Theory Manual 
Auricchio, F. and Taylor, R.L., “Shape-memory alloys: modeling and numerical 
simulations of the finite-strain superelastic behavior”, Computer Methods in Applie 
Mechanics and Engineering 143, 175-194 (1997). 
Back, S.Y., and Will, K.M., “A Shear-flexible Element with Warping for Thin-Walled 
Open Sections,” International Journal for Numerical Methods in Engineering, 43, 1173-1191 
(1998). 
Bahler AS:  The series elastic element of mammalian skeletal muscle.  Am J Physiol 
213:1560-1564, 1967. 
Bammann, D. J., and E.C. Aifantis, “A Model for Finite-Deformation Plasticity,” Acta 
Mechanica, 70, 1-13 (1987). 
Bammann, D. J., “Modeling the Temperature and Strain Rate Dependent Large 
Deformation of Metals,” Proceedings of the 11th US National Congress of Applied 
Mechanics, Tucson, AZ (1989). 
Bammann, D. J., and Johnson, G., “On the Kinematics of Finite-Deformation Plasticity,” 
Acta Mechanica 69, 97-117 (1987). 
Bammann, D.J., Chiesa, M.L., McDonald, A., Kawahara, W.A., Dike, J.J. and Revelli, 
V.D., “Predictions of Ductile Failure in Metal Structures,” in AMD-Vol.  107, Failure 
Criteria and Analysis in Dynamic Response, edited by.  H.E. Lindberg, 7-12 (1990). 
Bandak, F.A., private communications, U.S. Dept.  of Trans., Division of Biomechanics 
Research, 400 7th St., S.W.  Washington, DC 20590 (1991). 
Barlat and Lian, J., “Plastic Behavior and Stretchability of Sheet Metals, Part I: A Yield 
Function for Orthotropic Sheets Under Plane Stress Conditions,” International Journal of 
Plasticity, 5, 51-66 (1989). 
Barlat, F., Lege, D.J., and Brem, J.C., “A Six-Component Yield Function for Anisotropic 
Materials,” International Journal of Plasticity, 7, 693-712 (1991). 
Bathe, K. J., Finite Element Procedures in Engineering Analysis, Prentice-Hall (1982). 
Bathe, K. J., and Wilson, E.L., Numerical Methods in Finite Element Analysis, Prentice-
Hall (1976). 
Bathe, K.J., and Dvorkin, E.N., “A Continuum Mechanics Based Four Node Shell 
Element for General Nonlinear Analysis,” Int.  J. Computer-Aided Eng. and Software, 
Vol. 1, 77-88 (1984).
LS-DYNA Theory Manual 
References 
Bathe, K.-J. and Dvorkin, E.N. A four node plate bending element based on Mindlin-
Reissner plate theory and a mixed interpolation, Int.  J. Num.  Meth. Eng., 21, 367-383, 
1985. 
Batoz, J.L. and Ben Tahar, M. Evaluation of a new quadrilateral thin plate bending 
element, Int.  J. Num.  Meth. Eng., 18, 1644-1677, 1982. 
Battini, J., and Pacoste C., “Co-rotational Beam Elements with Warping Effects in 
Instability Problems,” Computational Methods in Applied Mechanical Engineering, 191, 
1755-1789, (2002).   
Bazeley, G.P., Cheung, W.K., Irons, B.M. and Zienkiewicz, O.C., “Triangular Elements 
in Plate Bending—Conforming and Nonconforming Solutions in Matrix Methods and 
Structural Mechanics,” Proc.  Conf.  on Matrix Methods in Structural Analysis, Rept.  
AFFDL-R-66-80, Wright Patterson AFB, 547-576 (1965). 
Belytschko, T., “Transient Analysis,” Structural Mechanics Computer Programs, edited 
by W. Pilkey, et.  al., University Press of Virginia, 255-276 (1974). 
Belytschko, T., and Bindeman, L. P., "Assumed Strain Stabilization of the Eight Node 
Hexahedral Element," Comp.  Meth.  Appl.  Mech.  Eng. 105, 225-260 (1993). 
Belytschko, T., and Hsieh, B.J., ”Nonlinear Transient Finite Element Analysis with 
Convected Coordinates,” Int.  J. Num.  Meths.  Engrg., 7, 255–271 (1973). 
Belytschko, T., and Leviathan, I., “Projection schemes for one-point quadrature shell 
elements,” Comp.  Meth.  Appl.  Mech. Eng., 115, 277-286 (1994). 
Belytschko, T., and Lin, J., “A New Interaction Algorithm with Erosion for EPIC-3”, 
Contract Report BRL-CR-540, U.S. Army Ballistic Research Laboratory, Aberdeen 
Proving Ground, Maryland (1985). 
Belytschko, T., Lin, J., and Tsay, C.S., “Explicit Algorithms for Nonlinear Dynamics of 
Shells,” Comp.  Meth.  Appl.  Mech.  Eng. 42, 225-251 (1984) [a]. 
Belytschko, T., Ong, J. S.-J., Liu, W.K. and Kennedy, J.M., “Hourglass Control in Linear 
and Nonlinear Problems”, Comput.  Meths.  Appl.  Mech.  Engrg., 43, 251–276 (1984b). 
Belytschko, T., Stolarski, H., and Carpenter, N., “A C0 Triangular Plate Element with 
One-Point Quadrature,” International Journal for Numerical Methods in Engineering, 
20, 787-802 (1984) [b].
References 
LS-DYNA Theory Manual 
Belytschko, T., Schwer, L., and Klein, M. J., “Large Displacement Transient Analysis of 
Space Frames,” International Journal for Numerical and Analytical Methods in 
Engineering, 11, 65-84 (1977). 
Belytschko, T., and Tsay, C.S., “Explicit Algorithms for Nonlinear Dynamics of Shells,” 
AMD, 48, ASME, 209-231 (1981). 
Belytschko, T., and Tsay, C.S., “WHAMSE: A Program for Three-Dimensional 
Nonlinear Structural Dynamics,” Report EPRI NP-2250, Project 1065-3, Electric Power 
Research Institute, Palo Alto, CA  (1982). 
Belytschko, T., and Tsay, C. S., “A Stabilization Procedure for the Quadrilateral Plate 
Element with One-Point Quadrature,” Int.  J. Num.  Method. Eng. 19, 405-419 (1983). 
Belytschko, T., Yen, H. R., and Mullen R., “Mixed Methods for Time Integration,” 
Computer Methods in Applied Mechanics and Engineering, 17, 259-175 (1979). 
Belytschko, T., “Partitioned and Adaptive Algorithms for Explicit Time Integration,” in 
Nonlinear Finite Element Analysis in Structural Mechanics, ed.  by Wunderlich, W. 
Stein, E, and Bathe, J. J., 572-584 (1980). 
Belytschko, T., Wong, B.L., and Chiang, H.Y., “Improvements in Low-Order Shell 
Elements for Explicit Transient Analysis,” Analytical and Computational Models of 
Shells, A.K. Noor, T. Belytschko, and J. Simo, editors, ASME, CED, 3,  383-398 (1989). 
Belytschko, T., Wong, B.L., and Chiang, H.Y., “Advances in One-Point Quadrature Shell 
Elements,” Comp.  Meths.  Appl.  Mech.  Eng., 96, 93-107 (1992). 
Belytschko, T., Wong, B. L., Plaskacz, E. J.,  "Fission - Fusion Adaptivity in Finite 
Elements for Nonlinear Dynamics of Shells," Computers and Structures, Vol.  33, 1307-
1323 (1989). 
Belytschko, T., Lu, Y.Y. and Gu, L., “Element-free Galerkin Methods,” Int.  J. Numer.  
Methods Engrg. 37, 229-256 (1994). 
Benson, D.J., “Vectorizing the Right-Hand Side Assembly in an Explicit Finite Element 
Program,” Comp.  Meths.  Appl.  Mech.  Eng., 73, 147-152 (1989). 
Benson, D. J., and Hallquist, J.O., “A Simple Rigid Body Algorithm for Structural 
Dynamics Program,” Int.  J. Numer.  Meth. Eng., 22 (1986). 
Benson, D.J., and Hallquist J.O., “A Single Surface Contact Algorithm for the 
Postbuckling Analysis of Shell Structures,” Comp.  Meths.  Appl.  Mech.  Eng., 78, 141-
163 (1990).
LS-DYNA Theory Manual 
References 
Benson, D. J., “Momentum Advection on a Staggered Mesh,” Journal of Computational 
Physics, 100, No.  1, (1992). 
Benson, D. J., “Vectorization Techniques for Explicit Arbitrary Lagrangian Eulerian 
Calculations,” Computer Methods in Applied Mechanics and Engineering (1992).  
Berstad, T., "Material Modelling of Aluminium for Crashworthiness Analysis", Dr.Ing.  
Dissertation, Department of Structural Engineering, Norwegian University of Science 
and Technology, Trondheim, Norway (1996). 
Berstad T., Hopperstad, O.S., and Langseth, M., “Elasto-Viscoplastic Consitiutive 
Models in the Explicit Finite Element Code LS-DYNA,” Proceedings of the Second 
International LS-DYNA Conference, San Francisco, CA (1994). 
Bischoff M. and Ramm E., “Shear deformable shell elements for large strains and 
rotations,” 
. Int.  J. Numer.  Methods, 40, 4427-4449 (1997). 
Blatz, P.J., and Ko, W.L., “Application of Finite Element Theory to the Deformation of 
Rubbery Materials,” Trans.  Soc.  of Rheology, 6, 223-251 (1962). 
Bodig, Jozsef and Benjamin A. Jayne, Mechanics of Wood and Wood Composites, 
Krieger Publishing Company, Malabar, FL (1993). 
Boeing, Boeing Extreme Mathematical Library BCSLIB-EXT User's Guide, The Boeing 
Company, Document Number 20462-0520-R4 (2000). 
Borrvall, T., Development and implementation of material tangent stiffnesses for 
material model 76 in LS-DYNA, ERAB-02:46, Engineering Research Nordic AB, 
Linköping (2002). 
Borrvall, T., Revision of the implementation of material 36 for shell elements in LS-
DYNA, ERAB Report E0307, Engineering Research Nordic AB, Linköping (2003). 
Björklund O., “Ductile Failure in High Strength Steel Sheets,” Linköping Studies in 
Science and Technology.  Dissertations No.  1579, ISSN 0345-7524 (2014). 
Brekelmans, W.A.M., Scheurs, P.J.G., and de Vree, J.H.P., “Continuum damage 
mechanics for softening of brittle materials”, Acta Mechanica, 93, 133-143, (1991). 
Brooks, A. N., and Hughes, T. J. R., “Streamline Upwind/Petrov-Galerkin Formulations 
for Convection Dominated Flows with Particular Emphasis on the Incompressible 
Navier-Stokes  Equations,” Computer Methods in Applied Mechanics and Engineering, 
32, 199-259, (1982).
References 
LS-DYNA Theory Manual 
Burton, D.E., et.  al., “Physics and Numerics of the TENSOR Code,” Lawrence 
Livermore National Laboratory, Internal Document UCID-19428 (July 1982). 
Cardoso, R.P.R. and Yoon J-W., “One point quadrature shell element with through-
thickness stretch, Computer Methods in Applied Mechanics and Engineering,” 194(9), 
1161-1199 (2005). 
Chang, F.K., and Chang, K.Y., “Post-Failure Analysis of Bolted Composite Joints in 
Tension or Shear-Out Mode Failure,” J. of Composite Materials, 21, 809-833 (1987).[a] 
Chang, F.K., and Chang, K.Y., “A Progressive Damage Model for Laminated 
Composites Containing Stress Concentration,” J. of Composite Materials, 21, 834-855 
(1987).[b] 
Chang, F.S., “Constitutive Equation Development of Foam Materials,” Ph.D. 
Dissertation, submitted to the Graduate School, Wayne State University, Detroit, 
Michigan (1995). 
Chang, F.S., J.O. Hallquist, D. X. Lu, B. K. Shahidi, C. M. Kudelko, and J.P. Tekelly,  
“Finite Element Analysis of Low Density High-Hystersis Foam Materials and the 
Application in the Automotive Industry,” SAE Technical Paper 940908, in Saftey 
Technology (SP-1041), International Congress and Exposition, Detroit, Michigan (1994). 
Chen, J.S., Pan, C., Wu, C.T. and Liu, W.K., “Reproducing Kernel Particle Methods for 
Large Deformation Analysis of Nonlinear Structures,” Comput.  Methods Appl.  Mech.  
Engrg. 139, 195-227 (1996). 
Chen, J.S. and Wu, C.T., “Generalized Nonlocal Meshfree Method in Strain 
Localization,” Proceeding of International Conference on Computational Engineering Science, 
Atlanta, Georiga, 6-9 October (1998).  
Chen, J.S. and Wang, H.P. “New Boundary Condition Treatmens in Meshfree 
Computation of Contact Problems,” Computer Methods in Applied Mechanics and 
Engineering, 187, 441-468, (2001a). 
Chen, J.S., Wu, C.T., Yoon, S. and You, Y. “A Stabilized Conforming Nodal Integration 
for Galerkin Meshfree Methods,” Int.  J. Numer.  Methods Engrg. 50, 435-466 (2001b). 
Chen, W.F., and Baladi, G.Y., Soil Plasticity: Theory and Implementation, Elesvier, New 
York, (1985).
LS-DYNA Theory Manual 
References 
Christensen, R.M. “A Nonlinear Theory of Viscoelasticity for Application to 
Elastomers,” Journal of Applied Mechanics, 47, American Society of Mechanical Engineers, 
762-768 (December 1980). 
Chung, K., and K. Shah, “Finite Element Simulation of Sheet Metal Forming for Planar 
Anisotropic Metals,” Int.  J. of Plasticity, 8, 453-476 (1992). 
Cochran, S.G., and Chan, J., “Shock Initiation and Detonation Models in One and Two 
Dimensions,” University of California, Lawrence Livermore National Laboratory, Rept.  
UCID-18024 (1979). 
Cohen, M., and Jennings, P.C., “Silent Boundary Methods for Transient Analysis”, in 
Computational Methods for Transient Analysis, T. Belytschko and T.J.R. Hughes, 
editors, North-Holland, New York, 301-360 (1983). 
Cook, R. D., Concepts and Applications of Finite Element Analysis, John Wiley and 
Sons, Inc.  (1974). 
Couch, R., Albright, E. and Alexander, “The JOY Computer Code,” University of 
California, Lawrence Livermore National Laboratory, Rept.  UCID-19688 (1983). 
Cray Research Inc., “CF77 Compiling System, Volume 4: Parallel Processing Guide,” 
SG-3074 4.0, Mendota Heights, MN (1990). 
Crisfield M.A., Non-linear Finite Element Analysis of Solids and Structures, Volume 2, 
Advanced Topics, John Wiley, New York (1997). 
DeBar, R. B., “Fundamentals of the KRAKEN Code,” Lawrence Livermore Laboratory, 
UCIR-760 (1974). 
Deshpande, V.S. and N.A. Fleck, “Isotropic Models for Metallic Foams,” Journal of the 
Mechanics and Physics of Solids, Vol.  48, 1253-1283, (2000). 
Dobratz, B.M., “LLNL Explosives Handbook, Properties of Chemical Explosives and 
Explosive Simulants,” University of California, Lawrence Livermore National 
Laboratory, Rept.  UCRL-52997 (1981). 
Duff, I. S., and Reid, J. K., "The Multifrontal Solution of Indefinite Sparse Symmetric 
Linear Equations," ACM Transactions of Mathematical Software, 9, 302-325 (1983). 
Dvorkin, E.N. and Bathe, K.J. “A continuum mechanics based four-node shell element 
for general nonlinear analysis,” International Journal for Computer-Aided Engineering 
and Software, 1, 77-88 (1984).
References 
LS-DYNA Theory Manual 
Englemann, B.E. and Whirley, R.G., “A New Explicit Shell Element Formulation for 
Impact Analysis,” In Computational Aspects of Contact Impact and Penetration, Kulak, 
R.F., and Schwer, L.E., Editors, Elmepress International, Lausanne, Switzerland, 51-90 
(1991). 
Englemann, B.E., Whirley, R.G., and Goudreau, G.L., “A Simple Shell Element 
Formulation for Large-Scale Elastoplastic Analysis,” In Analytical and Computational 
Models of Shells, Noor, A.K., Belytschko, T., and Simo, J.C., Eds., CED-Vol.  3, ASME, 
New York, New York (1989). 
Farhoomand, I., and Wilson, E.L., “A Nonlinear Finite Element Code for Analyzing the 
Blast Response of Underground Structures,” U.S. Army Waterways Experiment Station, 
Contract Rept.  N-70-1 (1970). 
Feng, W.W., Private communication, Livermore, CA (1993). 
Flanagan, D.P. and Belytschko, T., “A Uniform Strain Hexahedron and Quadrilateral 
and Orthogonal Hourglass Control,” Int.  J. Numer.  Meths. Eng. 17, 679-706 (1981) 
Fleck, J.T., “Validation of the Crash Victim Simulator,” I - IV, Report No.  DOT-HS-806 
279 (1981). 
Fleischer M., Borrvall T., and Bletzinger K-U., “Experience from using recently 
implemented enhancements for Material 36 in LS-DYNA 971 performing a virtual 
tensile test”, 6th European LS-DYNA Users Conference, Gothenburg, Sweden, 2007. 
“Fundamental Study of Crack Initiation and Propagation,” Author unknown, LLNL 
report, document received from LSTC (2003). 
Galbraith, P.C., M.J. Finn, S.R. MacEwen, et.al., "Evaluation of an LS-DYNA3D Model 
for Deep-Drawing of Aluminum Sheet", FE-Simulation of 3-D Sheet Metal Forming 
Processes in Automotive Industry, VDI Berichte, 894, 441-466 (1991).  
Ghanem RG, Spanos PD. Stochastic Finite Elements – A Spectral Approach, Springer-
Verlag, 1991, Revised Edition, Dover, 2003. 
Ginsberg, M. and Johnson, J.P., “Benchmarking the Performance of Physical Impact 
Simulation Software on Vector and Parallel Computers,” Proc.  of the Supercomputing 
88: Vol.  II, Science and Applications, Computer Society Press (1988). 
Gingold, R.A., and Monaghan, J.J., “Smoothed Particle Hydrodynamics: Theory and 
Application to Non-Spherical Stars,” Mon.  Not.  R. Astron.  Soc. 181, 375-389 (1977).
LS-DYNA Theory Manual 
References 
Ginsberg, M., and Katnik, R.B., “Improving Vectorization of a Crashworthiness Code,” 
SAE Technical Paper No.  891985, Passenger Car Meeting and Exposition, Dearborn, MI 
(1989). 
Giroux, E.D., “HEMP User's Manual,” University of California, Lawrence Livermore 
National Laboratory, Rept.  UCRL-51079 (1973). 
Govindjee, S., Kay G.J., and Simo, J.C., “Anisotropic Modeling and Numerical 
Simulation of Brittle Damage in Concrete,” Report Number UCB/SEM M-94/18, 
University of California at Berkeley, Department of Civil Engineering (1994). 
Govindjee, S., Kay G.J., and Simo, J.C., “Anisotropic Modeling and Numerical 
Simulation of Brittle Damage in Concrete,” International Journal for Numerical Methods in 
Engineering, Volume 38, pages 3611-3633 (1995). 
Green, A.E. and Naghdi, P.M., “A General Theory of Elastic-Plastic Continuum,” 
Archive for Rational Mechanics and Analysis, 18, 251 (1965). 
Groenwold, A.A. and Stander, N. An efficient 4-node 24 d.o.f. thick shell finite element 
with 5-point quadrature. Eng. Comput. 12(8), 723-747, 1995. 
Grimes, Roger, Lewis, John G., and Simon, Horst D., "A Shifted Block Lanczos 
Algorithm for Solving Sparse Symmetric Generalized Eigenproblems," SIAM Journal of 
Matrix Analyis and Applications, 15, 228-272 (1994). 
Guccione, J.,  A. McCulloch, and L. Waldman, "Passive Material Properties of Intact 
Ventricular Myocardium Determined from a Cylindrical Model," published in the 
ASME Journal of Biomechanical Engineering, 113, 42-55 (1991). 
Hallquist, J.O., “Preliminary User’s Manuals for DYNA3D and DYNAP (Nonlinear 
Dynamic Analysis of Solids in Three Dimension),” University of California, Lawrence 
Livermore National Laboratory, Rept.  UCID-17268 (1976) and Rev.  1 (1979).[a] 
Hallquist, J.O., “A Procedure for the Solution of Finite Deformation Contact-Impact 
Problems by the Finite Element Method,” University of California, Lawrence Livermore 
National Laboratory, Rept.  UCRL-52066 (1976). 
Hallquist, J.O., “A Numerical Procedure for Three-Dimensional Impact Problems,” 
American Society of Civil Engineering, Preprint 2956 (1977). 
Hallquist, J.O., “A Numerical Treatment of Sliding Interfaces and Impact,” in: K.C. Park 
and D.K. Gartling (eds.) Computational Techniques for Interface Problems, AMD, 30, 
ASME, New York (1978).
References 
LS-DYNA Theory Manual 
Hallquist, J.O., “NIKE2D: An Implicit, Finite-Element Code for Analyzing the Static and 
Dynamic Response of Two-Dimensional Solids,” University of California, Lawrence 
Livermore National Laboratory, Rept.  UCRL-52678 (1979).[b] 
Hallquist, J.O. (1998), LS-DYNA Theoretical Manual, May (1998). 
Hallquist, J.O., “User's Manual for DYNA2D— An Explicit Two-Dimensional 
Hydrodynamic Finite Element Code with Interactive Rezoning,” University of 
California, Lawrence Livermore National Laboratory, Rept.  UCID-18756 (1980). 
Hallquist, J.O., “User's Manual for DYNA3D and DYNAP (Nonlinear Dynamic 
Analysis of Solids in Three Dimensions),” University of California, Lawrence Livermore 
National Laboratory, Rept.  UCID-19156 (1981).[a] 
Hallquist, J. O., “NIKE3D: An Implicit, Finite-Deformation, Finite-Element Code for 
Analyzing the Static and Dynamic Response of Three-Dimensional Solids,” University 
of California, Lawrence Livermore National Laboratory, Rept.  UCID-18822 (1981).[b] 
Hallquist, J.O., “DYNA3D User's Manual (Nonlinear Dynamic Analysis of Solids in 
Three Dimensions),” University of California, Lawrence Livermore National 
Laboratory, Rept.  UCID-19156 (1982; Rev.  1: 1984; Rev.  2: 1986). 
Hallquist, J.O., “Theoretical Manual for DYNA3D,” University of California, Lawrence 
Livermore National Laboratory, Rept.  UCID-19401 (March, 1983). 
Hallquist, J.O., “DYNA3D User's Manual (Nonlinear Dynamic Analysis of Solids in 
Three Dimensions),” University of California, Lawrence Livermore National 
Laboratory, Rept.  UCID-19156 (1988, Rev.  4). 
Hallquist, J.O., “DYNA3D User's Manual (Nonlinear Dynamic Analysis of Solids in 
Three Dimensions),” Livermore Software Technology Corporation, Rept.  1007 (1990). 
Hallquist, J.O., LS-DYNA Keyword User’s Manual, version 970, Livermore Software 
Technology Corporation (April, 2003). 
Hallquist, J.O., Benson, D.J., and Goudreau, G.L., “Implementation of a Modified 
Hughes-Liu Shell into a Fully Vectorized Explicit Finite Element Code,” Proceedings of 
the International Symposium on Finite Element Methods for Nonlinear Problems, 
University of Trondheim, Trondheim, Norway (1985). 
Hallquist, J.O., and Benson, D.J., “A Comparison of an Implicit and Explicit 
Implementation of the Hughes-Liu Shell,” Finite Element Methods for Plate and Shell
LS-DYNA Theory Manual 
References 
Structures, T.J.R. Hughes and E. Hinton, Editors, 394-431, Pineridge Press Int., Swanea, 
U.K. (1986). 
Hallquist, J.O., and Benson, D.J., “DYNA3D User’s Manual (Nonlinear Dynamic 
Analysis of Solids in Three Dimensions),” University of California, Lawrence Livermore 
National Laboratory, Rept.  UCID-19156 (1986, Rev.  2). 
Hallquist, J.O. and Benson, D.J., “DYNA3D User’s Manual (Nonlinear Dynamic 
Analysis of Solids in Three Dimensions),” University of California, Lawrence Livermore 
National Laboratory, Rept.  UCID-19156 (1987, Rev.  3). 
Hallquist, J.O., Stillman, D.W., Hughes, T.J.R., and Tarver, C.,”Modeling of Airbags 
Using MVMA/DYNA3D,” LSTC Report (1990). 
Harten, A., “ENO Schemes with Subcell Resolution,” J. of Computational Physics, 83, 
148-184, (1989). 
Hashin, Z, “Failure Criteria for Unidirectional Fiber Composites,” Journal of Applied 
Mechanics, 47, 329 (1980). 
Herrmann, L.R. and Peterson, F.E., “A Numerical Procedure for Viscoelastic Stress 
Analysis,” Seventh Meeting of ICRPG Mechanical Behavior Working Group, Orlando, 
FL, CPIA Publication No.  177 (1968). 
Hill A.V., "The heat of shortening and the dynamic constants of muscle,"  Proc Roy Soc 
B126:136-195, (1938). 
Hill, R., “A Theory of the Yielding and Plastic Flow of Anisotropic Metals,” Proceedings 
of the Royal Society of London, Series A., 193, 281 (1948). 
Hill, R. “Consitiutive Modeling of Orthotropic Plasticity in Sheet Metals,” Journal of 
Mechanics and Physics of Solids, 38, Number 3, 405-417 (1999). 
Holmquist, T.J., G.R. Johnson, and W.H. Cook, "A Computational Constitutive Model 
for Concrete Subjected to Large Strains, High Strain Rates, and High Pressures, pp.  591-
600, (1993). 
Holtz R.D.,  W. D. Kovacs, “ An Introduction to Geotechnical Engineering”, Prentice 
Hall, Inc. New Jersey, 1981 
Hopperstad, O.S. and Remseth, S., “A Return Mapping Algorithm for a Class of Cyclic 
Plasticity Models,” International Journal for Numerical Methods in Engineering, 38, 549-564 
(1995).
References 
LS-DYNA Theory Manual 
Hughes, T.J.R., The Finite Element Method, Linear Static and Dynamic Finite Element 
Analysis, Prentice-Hall Inc., Englewood Cliffs, NJ (1987). 
Hughes, T.J.R., “Generalization of Selective Integration Procedures to Anisotropic and 
Nonlinear Media,” Int.  J. Numer.  Meth. Eng. 15, 9 (1980). 
Hughes, T.J.R. and Carnoy, E., “Nonlinear Finite Element Shell Formulation Accounting 
for Large Membrane Strains,” AMD-Vol.48, ASME, 193-208 (1981). 
Hughes, T.J.R. and Liu, W.K., “Nonlinear Finite Element Analysis of Shells:  Part I.  
Two-Dimensional Shells.” Comp.  Meths.  Appl.  Mechs. 27, 167-181 (1981). 
Hughes, T.J.R. and Liu, W.K., “Nonlinear Finite Element Analysis of Shells:  Part II. 
Three-Dimensional Shells.” Comp.  Meths.  Appl.  Mechs. 27, 331-362 (1981). 
Hughes, T.J.R., Liu,W.K., and Levit, I., “Nonlinear Dynamics Finite Element Analysis of 
Shells.” Nonlinear Finite Element Analysis in Struct.  Mech., Eds.  W. Wunderlich, E. 
Stein, and K.J. Bathe, Springer-Verlag, Berlin, 151–168 (1981). 
Hughes, T.J.R., Taylor, R. L., Sackman, J. L., Curnier, A.C., and Kanoknukulchai, W., “A 
Finite Element Method for a Class of Contact-Impact Problems,” J. Comp.  Meths.  
Appl.  Mechs. Eng. 8, 249-276 (1976). 
Hughes, T.J.R., and Winget, J., “Finite Rotation Effects in Numerical Integration of Rate 
Constitutive Equations Arising in Large-Deformation Analysis,” Int.  J. Numer.  Meths. 
Eng., 15, 1862-1867, (1980). 
Hulbert, G.M. and Hughes, T.J.R., “Numerical Evaluation and Comparison of 
Subcycling Algorithms for Structural Dynamics,” Technical Report, DNA-TR-88-8, 
Defense Nuclear Agency, Washington, DC (1988). 
Ibrahimbegovic, A. and Wilson, E.L. A unified formulation for triangular and 
quadrilateral flat shell finite elements with six nodal degrees of freedom, Comm.  Applied 
Num.  Meth, 7, 1-9, 1991. 
Isenberg, J., D.K. Vaughn, and I. Sandler, "Nonlinear Soil-Structure Interaction," EPRI 
Report MP-945, Weidlinger Associates, December (1978). 
Jabareen,  M.,  and  Rubin,  M.B.,  A  Generalized  Cosserat  Point  Element  (CPE)  for 
Isotropic Nonlinear Elastic Materials including Irregular 3-D Brick and Thin Structures, 
J. Mech.  Mat.  And Struct., Vol 3-8, 1465-1498 (2008).
LS-DYNA Theory Manual 
References 
Jabareen,  M.,  Hanukah,  E.  and  Rubin,  M.B.,  A  Ten  Node  Tetrahedral  Cosserat  Point 
Element (CPE) for Nonlinear Isotropic Elastic Materials, J. Comput.  Mech.  52, 257-285 
(2013). 
Jaumann, G. “Geschlossenes System Physikalischer und Chemischer Differentialdesefz, 
Sitz Zer. Akad.  Wiss.  Wein, (IIa), 120, 385 (1911). 
Johnson, G.C. and Bammann D.J., “A Discussion of Stress Rates in Finite Deformation 
Problems" International Journal of Solids and Structures, 20, 725-737 (1984). 
Johnson, G.R. and Cook,W. H., “A Constitutive Model and Data for Metals Subjected to 
Large Strains, High Strain Rates and High Temperatures,” presented at the Seventh 
International Symposium on Ballistics, The Hague, The Netherlands, April (1983). 
Johnson, G.R. and T.J. Holmquist, "An Improved Computational Model for Brittle 
Materials" in High-Pressure Science and Technology - 1993 American Institute of 
Physics Conference Proceedings 309 (c 1994) pp.981-984  ISBN 1-56396-219-5. 
Johnson, C., Navert, U., and Pitkaranta, J., “Finite Element Methods for Linear 
Hyperbolic Problems,” Computer Methods in Applied Mechanics and Engineering, 45, 
285-312, (1984). 
Jones, N., “Structural Aspects of Ship Collisions,” Chapter 11, in Structural 
Crashworthiness, Eds.  N. Jones and T Wierzbicki, Butterworths, London, 308-337 
(1983). 
Jones, R.M., Mechanics of Composite Materials, Hemisphere Publishing Co., New York 
(1975). 
Ju J.W., “Energy-Based Coupled Elastoplastic Damage Models at Finite Strains”, J. of 
Eng Mech., Vol 115, No 11, Nov 1989.  
Karypis, G., and Kumar V., "METIS: A Software Package for Partitioning Unstructured 
Graphs, Partitioning Meshes, and Computing Fill-Reducing Orderings of Sparse 
Matrices," Department of Computer Science, University of Minnesota (1998). 
Katz, J., and Maskew, B., “Unsteady Low-Speed Aerodynamic Model for Complete 
Aircraft Configurations,” Journal of Aircraft 25, 4 (1988). 
Kenchington, G. J., “A Non-Linear Elastic Material Model for DYNA3D,” Proceedings 
of the DYNA3D Users Group Conference, September 1988, published by Boeing 
Computer Services (Europe) Limited.
References 
LS-DYNA Theory Manual 
Kennedy, J. M., Belytschko,T., and Lin, J. I., “Recent Developments in Explicit Finite 
Element Techniques and their Applications to Reactor Structures,” Nuclear Engineering 
and Design 97, 1-24 (1986). 
Kim, N., Seo, K., and Kim, M., “Free Vibration and Spatial Stability of Non-symmetric 
Thin-Walled Curved Beams with Variable Curvatures,” International Journal of Solids and 
Structures, 40, 3107-3128, (2003).  
Klisinski M., “Degradation and Plastic Deformation of Concrete”, Ph.D. thesis, Polish 
Academy of Sciences, 1985, IFTR report 38. 
Kosloff, D. and Frazier, G.A.,“Treatment of Hourglass Patterns in Low Order Finite 
Element 
Codes,” Int.  J. Numer.  Anal.  Meth.  Geomech. 2, 57-72 (1978) 
Kretschmann, D. E., and David W. Green, “Modeling Moisture Content-Mechanical 
Property Relationships for Clear Southern Pine,” Wood and Fiber Science, 28(3), pp.  
320-337 (1996). 
Kreyszig, E., Advanced Engineering Mathematics, John Wiley and Sons, New York, 
New York (1972). 
Krieg, R.D.,”A Simple Constitutive Description for Cellular Concrete,” Sandia National 
Laboratories, Albuquerque, NM, Rept.  SC-DR-72-0883 (1972). 
Krieg, R.D. and Key, S.W., Implementation of a Time Dependent Plasticity Theory into 
Structural Computer Programs, Vol.  20 of Constitutive Equations in Viscoplasticity: 
Computational and Engineering Aspects (American Society of Mechanical Engineers, 
New York, N.Y., 1976), 125-137. 
Kumar, P., Nukala, V. V., and White, D. W., “A Mixed Finite Element for Three-
dimensional Nonlinear Analysis of Steel Frames,” Computational Methods in Applied 
Mechanical Engineering, 193, 2507-2545, (2004). 
Lancaster, P. and Salkauskas, K., “Surfaces generated by moving least squares 
methods”, Math.  Comput. 37, 141-158, (1981). 
Landshoff, R., “A Numerical Method for Treating Fluid Flow in the Presence of 
Shocks,” Los Alamos Scientific Laboratory, Rept.  LA-1930 (1955). 
Lee, E.L. and Tarver, C.M., “Phenomenological Model of Shock Initiation in 
Heterogeneous Explosives,” Phys.  of Fluids, 23, 2362 (1980).
LS-DYNA Theory Manual 
References 
Lemaitre, J., A Course on Damage Mechanics.  Springer-Verlag, (1992). 
Lemmen, P.P.M and Meijer, G.J., “Failure Prediction Tool Theory and User Manual,” 
TNO Building and Construction Research, The Netherlands, Rept.  2000-CMC-R0018, 
(2001).  
Lewis B.A., “Developing and Implementing a Road Side Safety Soil Model into LS-
DYNA”,  FHWA Research and Development Turner-Fairbank Highway Research 
Center.  Oct, 1999.  
Librescu, L. Qin, Z., and Ambur D.R., “Implications of Warping Restraint on Statics and 
Dynamics of Elastically Tailored Thin-Walled Composite Beams,” International Journal of 
Mechanical Sciences, 45, 1247-1267 (2003).  
Liu, Joseph W. H., "Modification of the Minimum-Degree Algorithm by Multiple 
Elimination," ACM Transactions on Mathematical Software, 11, 141-153 (1985). 
Liu, W.K. and Belytschko, T., “Efficient Linear and Nonlinear Heat Conduction with a 
Quadrilateral Element,” Int.  J. Num.  Meths.  Engrg., 20, 931–948 (1984). 
Liu, W.K., Belytschko, T., Ong, J.S.J. and Law, E., “Use of Stabilization Matrices in 
Nonlinear Finite Element Analysis,” Engineering Computations, 2, 47–55 (1985). 
Liu, W.K., Lecture Notes on Nonlinear Finite Element Methods, Northwestern 
University, (1983, revised in 1992). 
Liu, W.K., Guo, Y., Tang, S. and Belytschko T., “A Multiple-Quadrature Eight-node 
Hexahedral Finite Element for Large Deformation Elastoplastic Analysis,” Comput.  
Meths.  Appl.  Mech.  Engrg., 154, 69–132 (1998). 
Liu, W.K., Hu, Y.K., and Belytschko, T., “Multiple Quadrature Underintegrated Finite 
Elements,” Int.  J. Num.  Meths.  Engrg., 37, 3263–3289 (1994). 
Liu, W. K., Chang, H., and Belytschko, T., “Arbitrary Lagrangian-Eulerian Petrov-
Galerkin Finite Elements for Nonlinear Continua,” Computer Methods in Applied 
Mechanics and Engineering, to be published. 
Liu, W.K., Jun, S. and Zhang, Y.F., “Reproducing Kernel Particle Method,” Int.  J. 
Numer.  Methods Fluids 20, 1081-1106 (1995). 
Lucy, L.B., “Numerical Approach to Testing the Fission Hyphothesis,” Astron.  J. 82, 
1013-1024 (1977).
References 
LS-DYNA Theory Manual 
Lysmer, J. and Kuhlemeyer, R.L., “Finite Dynamic Model for Infinite Media”, J. Eng.  
Mech.  Div.  ASCE, 859-877 (1969). 
MacNeal R.H. and Harder R.L., “A Proposed Standard Set of Problems to Test Finite 
Element Accuracy,” Finite Elements Anal.  Des., (1985,  3–20 (1985). 
Maenchen, G. and Sack, S., “The Tensor Code,” Meth.  Comp.  Phys. 3, (Academic 
Press), 181-263 (1964). 
Maffeo, R., “TRANCITS Program User’s Manual,” General Electric Company, 
Cincinnati, OH, NASA Report CR-174891, (1985). 
Maffeo, R., “Burner Liner Thermal/Structural Load Modeling,” General Electric 
Company, Cincinnati, OH, NASA Report CR-174892, (1984). 
Maker, B. N., Private communication, Lawrence Livermore National Laboratory.  Dr. 
Maker programmed and implemented the compressible Mooney-Rivlin rubber model. 
Marchertas, A. H., and Belytschko,T. B., “Nonlinear Finite Element Formulation for 
Transient Analysis of Three Dimensional Thin Structures,” Report ANL-8104, LMFBR 
Safety, Argonne National Laboratory, Argonne, IL (1974). 
Margolin, L. G., personal communication to D. Benson (1989). 
Maskew, B., “Program VSAERO Theory Document,” NASA CR-4023 (1987). 
Matthies, H., and G. Strang, The Solution of Nonlinear Finite Element Equations, Int., 
Journal for Numerical Methods in Engineering, 14, No.  11, 1613-1626. 
Matzenmiller, A., and Schweizerhof, K., “Crashworthiness Simulatios of Composite 
Structures - A First Step with Explicit Time Integration,” Nonlinear Computational 
mechanics - A State of the Art, edited by P.W. Wriggers, et.  al., Springer-Verlag, (1991). 
Mauldin, P.J., R.F. Davidson, and R.J. Henninger, “Implementation and Assessment of 
the Mechanical-Threshold-Stress Model Using the EPIC2 and PINON Computer 
Codes,”  Report LA-11895-MS, Los Alamos National Laboratory (1990). 
McGlaun, personal communication to D. Benson, Sandia National Laboratories, (1990). 
McGlaun, J. M.,  Thompson, S. L.,  and Elrick, M. G., ”CTH: A Three-Dimensional Shock 
Wave Physics Code,” Proc.  of the 1989 Hypervelocity Impact Symposium (1989). 
Mindlin, R.D., “Influence of Rotary Inertia and Shear on Flexural Motions of Isotropic, 
Elastic Plates,” J. Appl.  Mech. 18, 31-38 (1951).
LS-DYNA Theory Manual 
References 
Mizukami, A., and Hughes, T. J. R., “A Petrov-Galerkin Finite Element Method for 
Convection Dominated Flows: An Accurate Upwinding Technique for Satisfying the 
Maximum Principle,” Computer Methods in Applied Mechanics and Engineering, Vol.  
50, pp.  181-193 (1985). 
Monaghan, J.J., and Gingold, R.A., “Shock Simulation by the Particle Method of SPH,”  
Journal of Computational Physics, 52, 374-381 (1983). 
Murray Y.D., “Modeling Rate Effects in Rock and Concrete”, Proceedings of the 8th 
International Symposium on Interaction of the Effects of Munitions with Structures, 
Defense Special Weapons Agency,  McLean VA, USA, (1997). 
Murray, Y. D., “Modeling Rate Effects in Rock and Concrete,” Proceedings of the 8th 
International Symposium on Interaction of the Effects of Munitions with Structures, 
Defense Special Weapons Agency, McLean, VA, USA, (1997). 
Murray, Y.D., Users Manual for Transversely Isotropic Wood Model, aptek technical 
report to fhwa (to be published), (2002). 
Murray, Y.D., and J. Reid, Evaluation of Wood Model for Roadside Safety Applications, 
aptek technical report to fhwa (to be puslished), (2002). 
Nagtegaal, J.C., Parks, D.M., and Rice J.R., “On Numerically Accurate Finite Element 
Solution in the Fully Plastic Range”, Computer Methods in Applied Mechanics and 
Engineering, 4, 153 (1974). 
Newman, W.M., and Sproull, R.F., Principles of Interactive Computer Graphics, 
McGraw-Hill, New York (1979). 
Newmark, N., “A Method of Computation for Structural Dynamics,” Journal of the 
Engineering Mechanics Division, Proceedings of the American Society of Civil 
Engineers, 67-94 (1959). 
Neilsen, M.K., Morgan, H.S., and Krieg, R.D., “A Phenomenological Constitutive Model 
for Low Density Polyurethane Foams,” Rept.  SAND86-2927, Sandia National 
Laboratories, Albuquerque, NM (1987). 
Noh, W.F.,  Meth.  Comp.  Phys. 3, (Academic Press)  (1964). 
Noh, W.F., “Numerical Methods in Hydrodynamic Calculations,” University of 
California, Lawrence Livermore National Laboratory, Rept.  UCRL-52112 (1976). 
Oden, J.T, P. Devloo, and T. Strouboulis, "Adaptive Finite Element Methods for the 
Analysis of Inviscid Compressible Flow:  Part I.  Fast Refinement/Unrefinement and
References 
LS-DYNA Theory Manual 
Moving Mesh Methods for Unstructured Meshes," Computer Methods in Applied 
Mechanics and Engineering, 59, 327-362 (1986). 
Ogden, R.W., Non-Linear Elastic Deformations, Ellis Horwood Ltd., Chichester, Great 
Britian (1984). 
Okuda T., Yamamae Y. and Yasuki T., Request for MAT126 Modification, Microsoft 
Power Point presentation, Toyota Communication Systems and Toyota Motor 
Corporation, 2003. 
Oliver, J., “A Consistent Characteristic Length of  Smeared Cracking Models,” 
International Journal for Numerical Methods in Engineering, 28, 461-474 (1989). 
Rajendran, A.M.,"Material Failure Models", in Material Behavior at High Strain Rates, 
Course Notes, Computational Mechanics Associates, Monterey, CA, 424 (1989). 
Papadrakakis, M., “A Method for the Automated Evaluation of the Dynamic Relaxation 
Parameters,” Comp.  Meth.  Appl.  Mech.  Eng. 25, 35-48 (1981).  
Phoon KK, Huang SP, Quek ST. Implementation of Karhunen–Loeve expansion for 
simulation using a wavelet-Galerkin scheme.  Probabilist Eng Mech 2002;17(3):293–303. 
(2002a)  
Phoon KK, Huang SP, Quek ST. Simulation of second-order processes using Karhunen–
Loeve expansion.  Comput Struct 2002; 80(12):1049–60. (2002b)  
Phoon KK, Huang HW, Quek ST. Simulation of strongly non-Gaussian processes using 
Karhunen–Loeve expansion, Probabilistic Engineering Mechanics 20 (2005) 188–198. 
Pian, T.H.H., and Sumihara, K., “Rational Approach for Assumed Stress Elements,” Int.  
J. Num.  Meth. Eng., 20, 1685-1695 (1985). 
Prokic, A., “New Warping Function for Thin-Walled Beams.  I:  Theory,” Journal of 
Structural Engineering, 122, 1437-1442, (1994). 
Przemieniecki, J. S., Theory of Matrix Structural Analysis, McGraw-Hill Book Company, 
New York, NY (1986). 
Reid, S.R. and C. Peng, “Dynamic Uniaxial Crushing of Wood,” Int.  J. Impact 
Engineering, Vol.  19, No.  5-6, pp.  531-570, (1997). 
Reyes, A., O.S. Hopperstad, T. Berstad, and M. Langseth, “Implementation of a Material 
Model for Aluminium Foam in LS-DYNA”, Report R-01-02, Restricted, Department of 
Structural Engineering, Norwegian University of Science and Technology, (2002).
LS-DYNA Theory Manual 
References 
Richards, G.T., “Derivation of a Generalized von Neumann Pseudo-Viscosity with 
Directional Properties,” University of California, Lawrence Livermore National 
Laboratory, Rept.  UCRL-14244 (1965). 
Richtmyer, R.D., and Morton, K.W., Difference Equations for Initial-Value Problems, 
Interscience Publishers, New York (1967). 
Sandler, I.S., and D. Rubin, “An Algorithm and a modular subroutine for the cap 
model,” Int.  J. Numer.  Analy.  Meth.  Geomech., 3, 173-186 (1979). 
Schwer, L.E., Cheva, W., and Hallquist, J.O., “A Simple Viscoelastic Model for Energy 
Absorbers Used in Vehicle-Barrier Impacts,” In Computational Aspects of Contact 
Impact and Penetration, Kulak, R.F., and Schwer, L.E., Editors, Elmepress International, 
Lausanne, Switzerland, 99-117 (1991). 
Shapiro, A.B., “TOPAZ3D - A Three Dimensional Finite Element Heat Transfer Code,” 
University of California, Lawrence Livermore National Laboratory, Report UCID-20481 
(1985). 
Shapiro, A.B., “REMAP: a Computer Code That Transfers Node Information Between 
Dissimilar Grids,” Lawrence Livermore National Laboratory, UCRL-ID-104090, (1990). 
Shkolnikov, M.B. Private Communication (1990-1991). 
Simo, J.C. and Govindjee, S., ``Exact Closed-Form Solution of the Return Mapping 
Algorithm in Plane Stress Elasto-Viscoplasticity," Engineering Computations, 5, 254-258 
(1988). 
Simo, J.C. and Hughes, T.J.R. “On the variational foundations of assumed strain 
methods,” Journal of Applied Mechanics, 53, 1685-1695 (1986). 
Simo, J.C., Ju, J.W., “Stress and Strain Based Continuum Damage Models”, Parts I & II, 
Int.  J. of Solids and Structures, Vol 23, No 7, (1987). 
Simo, J.C., Ju, J.W., Pister, K.S., and Taylor, R.L. “An Assessment of the Cap Model:  
Consistent Return Algorithms and Rate-Dependent Extension,” J. Eng.  Mech., 114, 
No.  2, 191-218 (1988a).  
Simo, J.C., Ju, J.W., Pister, K.S., and Taylor, R.L. “Softening Response, Completeness 
Condition, and Numerical Algorithms for the Cap Model,” Int. J. Numer.  Analy.  Meth. 
Eng.  (1990).
References 
LS-DYNA Theory Manual 
Simo, J.C. and Taylor, R.L., “A Return Mapping Algorithm for Plane Stress 
Elastoplasticity,” International Journal for Numerical Methods in Engineering, 22, 649-670 
(1986). 
Steinberg, D.J. and Guinan, M.W., “A High-Strain-Rate Constitutive Model for Metals,” 
University of California, Lawrence Livermore National Laboratory, Rept.  UCRL-80465 
(1978). 
Stillman, D. W., and Hallquist, J. O., “LS-INGRID: A Pre-Processor and Three-
Dimensional Mesh Generator for the Programs LS-DYNA, LS-NIKE3D, and 
TOPAZ3D,” Version 3.1, Livermore Software Technology Corporation (1992). 
Stojko, S., privated communication, NNC Limited, Engineering Development Center 
(1990). 
Stolarski, H., and Belytschko, T., “Shear and Membrane Locking in Curved Elements,” 
Comput.  Meths.  Appl.  Mech.  Engrg., 41, 279–296 (1983). 
Stone, C.M., Krieg, R.D., and Beisinger, Z.E., “Sancho, A Finite Element Computer 
Program for the Quasistatic, Large Deformation, Inelastic Response of Two-
Dimensional Solids,” Sandia Report, SAND 84-2618, UC-32, Albuquerque, NM (1985). 
Storakers, B., “On Material Representation and Constitutive Branching in Finite 
Compressible Elasticity”, Royal Institute of Technology, Stockholm Sweden, (1985). 
Sturt, R.M.V., and B.D. Walker, J.C. Miles, A. Giles, and N. Grew,  “Modelling the 
Occupant in a Vehicle Context-An Integrated Approach,” 13th International ESV 
Conference, Paris, November 4-7 (1991). 
Sussman, T. and Bathe, K.J., “A Finite Element Formulation for Nonlinear Incompressi-
ble Elastic and Inelastic Analysis,” Computers & Structures, 26, Number 1/2, 357-409 
(1987). 
Tarver, C.M., and Hallquist, J.O., “Modeling of Two-Dimensional Shock Initiation and 
Detonation Wave Phenomena in PBX 9404 and LX-17,” University of California, 
Lawrence Livermore National Laboratory, Rept.  UCID84990 (1981). 
Taylor, R.L. and Simo, J.C. Bending and membrane elements for the analysis of thick 
and thin shells, Proc.  of NUMETA Conference, Swansea, 1985. 
Taylor, R.L., Finite element anlysis of linear shell problems, in Whiteman, J.R. (ed.), 
Proc.  of the Mathematics in Finite Elements and Applications, Academic Press, New York, 
191-203 (1987).
LS-DYNA Theory Manual 
References 
Taylor, L.M., and Flanagan, D.P., “PRONTO3D A Three-Dimensional Transient Solid 
Dynamics Program,” Sandia Report: SAND87-1912, UC-32 (1989). 
Thompson, S. L., “CSQ -- A Two Dimensional Hydrodynamic Program with Energy 
Flow and Material Strength,” Sandia Laboratories, SAND74-0122 (1975). 
Thompson, R., L., and Maffeo, R. L., “A Computer Analysis Program for Interfacing 
Thermal and Structural Codes,” NASA Lewis Research Center, Report NASA-TM-
87021 (1985). 
Trefethen, L.N., “Group Velocity in Finite Difference Schemes,” SIAM Review, 24, No.  
2 (1982). 
Tsai, S.W., and Wu, E.M., “A General Theory of Strength for Anisotropic Materials,” 
Journal of Composite Materials, 58-80 (1971). 
Tuler, F.R. and B.M. Butcher, "A Criterion for the Time Dependence of Dynamic 
Fracture,"  The International Journal of Fracture Mechanics, 4, No.  4 (1968).  
Turk M, Pentland A. Eigenfaces for Recognition, Journal of Cognitive Neuroscience, 
1991; 3(1):71-86. 
Turkalj, G. Brnic, J., and Prpic-Orsic J., “Large Rotation Analysis of Elastic Thin-Walled 
Beam-Type Structures Using ESA Approach,” Computers & Structures, 81, 1851-1864, 
(2003). 
Underwood, P., “Dynamic Relaxation,” Computational Method for Transient Analysis, 
Belytschko, T., and Hughes, T.J.R., Eds., 1, 245-263, (1986).   
Van Leer, B., “Towards the Ultimate Conservative Difference Scheme.  IV. A New 
Approach to Numerical Convection,” Journal of Computational Physics, 23, 276-299 
(1977). 
Vawter, D., "A Finite Element Model for Macroscopic Deformation of the Lung," 
published in the Journal of Biomechanical Engineering, 102, 1-7, (1980). 
von Neumann, J., and Richtmyer, R.D., “A Method for the Numerical Calculation of 
Hydrodynamical Shocks,” J. Appl.  Phys., 21, 232 (1950). 
Walker, B.D., and P.R.B. Dallard, “An integrated Approach to Vehicle Crashworthiness 
and Occupant Protection Systems”, SAE International Congress and Exposition, Detroit, 
Michigan, (910148), February 25-March 1 (1991).
References 
LS-DYNA Theory Manual 
Walker, H.F., Numerical Solution of Nonlinear Equations, University of California, 
Lawrence Livermore National Laboratory, Rept.  UCID-18285 (1979). 
Wang, J. T., and O. J. Nefske, “A New CAL3D Airbag Inflation Model,” SAE paper 
880654, (1988). 
Wang, J. T., private communication (1992). 
Wang, J.T., "An Analytical Model for an Airbag with a Hybrid Inflator", Publication 
R&D 8332, General Motors Development Center, Warren, MI (1995). 
Wang, J.T., "An Analytical Model for an Airbag with a Hybrid Inflator", AMD-Vol.  210, 
BED 30, ASME, 467-497  (1995). 
Warsi, Z. U. A., “Basic Differential Models for Coordinate Generation,” in Symposium 
on the Numerical Generation of Curvilinear Coordinate Systems, Nashville, Tenn.  
(1982).  
Whirley, R. G., Hallquist, J. O., and Goudreau, G. L., “An Assessment of Numerical 
Algorithms for Plane Stress and Shell Elastoplasticity on Supercomputers,”  Engineering 
Computations, 6,  116-126 (June, 1989). 
Wilkins, M.L., “Calculations of Elastic Plastic Flow,” Meth.  Comp.  Phys., 3, (Academic 
Press), 211-263 (1964). 
Wilkins, M. L., “Calculation of Elastic-Plastic Flow,” University of California, Lawrence 
Livermore National Laboratory, Rept.  UCRL-7322, Rev.  I (1969). 
Wilkins, M.L., “Use of Artificial Viscosity in Multidimensional Fluid Dynamic 
Calculations,” J. Comp.  Phys. 36, 281 (1980). 
Wilkins, M.L., Blum, R.E., Cronshagen, E., and Grantham, P., “A Method for Computer 
Simulation of Problems in Solid Mechanics and Gas Dynamics in Three Dimensions and 
Time,” University of California, Lawrence Livermore National Laboratory, Rept.  
UCRL-51574 (1974). 
Wilson, E.L., Three Dimensional Static and Dynamic Analysis of Structures, A 
publication of Computers and Structures, Inc., Berkeley, California, [1996-2000]. 
Winslow, A. M., “Equipotential Zoning of Two-Dimensional Meshes,” Lawrence 
Radiation Laboratory, UCRL-7312 (1963). 
Winslow, A. M., “Equipotential Zoning of The Interior of a Three-Dimensional Mesh,” 
Report to LSTC (1990).
LS-DYNA Theory Manual 
References 
Winters, J.M., "Hill-based muscle models:  A systems engineering perspective,"  In 
Multiple Muscle Systems:  Biomechanics and Movement Organization, JM Winters and 
SL-Y Woo eds, Springer-Verlag (1990). 
Winters J.M. and Stark L., "Estimated mechanical properties of synergistic muscles 
involved in movements of a variety of human joints,":  J Biomechanics 21:1027-1042, 
(1988). 
Woodruff, J.P., “KOVEC User’s Manual,” University of California, Lawrence Livermore 
National Laboratory, Rept.  UCRL-51079 (1973). 
Yen, C.F. and Caiazzo, A, “Innovative Processing of Multifunctional Composite Armor 
for Ground Vehicles,” ARL-CR-484, U.S. Army Research Laboratory, Aberdeen Proving 
Ground, MD, (2001). 
Yunus, S.M., Pawlak, T.P., and Cook, R.D., “ Solid Elements with Rotational Degrees of 
Freedom, Part I-Hexahedron Elements,” To be published, (1989). 
Zajac F.E., "Muscle and tendon:  Properties, models, scaling, and application to 
biomechanics and motor control, "CRC Critical Reviews in Biomedical Engineering 
17(4):359-411, (1989).
References 
LS-DYNA Theory Manual

Corporate Address 
Livermore Software Technology Corporation 
P.  O.  Box 712 
Livermore, California 94551-0712 
Support Addresses 
Livermore Software Technology Corporation
7374 Las Positas Road 
Livermore, California 94551 
Tel:  925-449-2500     Fax:  925-449-2507 
Email:  sales@lstc.com 
Website:  www.lstc.com 
Disclaimer 
Technology 
Software 
Livermore 
Corporation 
1740 West Big Beaver Road 
Suite 100 
Troy, Michigan  48084 
Tel:  248-649-4728     Fax:  248-649-6328 
Copyright © 1992-2017 Livermore Software Technology Corporation.  All Rights Reserved. 
LS-DYNA®, LS-OPT® and LS-PrePost® are registered trademarks of Livermore Software 
Technology Corporation in the United States.  All other trademarks, product names and 
brand names belong to their respective owners. 
LSTC reserves the right to modify the material contained within this manual without prior 
notice. 
The information and examples included herein are for illustrative purposes only and are 
not intended to be exhaustive or all-inclusive.  LSTC assumes no liability or responsibility 
whatsoever for any direct of indirect damages or inaccuracies of any type or nature that 
could be deemed to have resulted from the use of this manual. 
Any  reproduction,  in  whole  or  in  part,  of  this  manual  is  prohibited  without  the  prior
LS-DYNA MULTIPHYSICS USER’S MANUAL 
INTRODUCTION 
In this manual, there are three main solvers: a compressible flow solver, an incompressible 
flow solver, and an electromagnetism solver.  Each of them implements coupling with the 
structural solver in LS-DYNA. 
The keywords covered in this manual fit into one of three categories.  In the first category 
are the keyword cards that provide input to each of the multiphysics solvers that in turn 
couple with the structural solver.  In the second category are keyword cards involving 
extensions to the basic solvers.  Presently, the chemistry and stochastic particle solvers are 
the two solvers in this category, and they are used in conjunction with the compressible 
flow solver discussed below.  In the third category are keyword cards for support facilities.  
A volume mesher that creates volume tetrahedral element meshes from bounding surface 
meshes is one of these tools.  Another is a new data output mechanism for a limited set of 
variables  from  the  solvers  in  this  manual.    This  mechanism  is  accessed  through  *LSO 
keyword cards. 
The  CESE  solver  is  a  compressible  flow  solver  based  upon  the  Conservation  Ele-
ment/Solution  Element  (CE/SE)  method,  originally  proposed  by  Chang  of  the  NASA 
Glenn Research Center.  This method is a novel numerical framework for conservation 
laws.  It has many non-traditional features, including a unified treatment of space and time, 
the introduction of separate conservation elements (CE) and solution elements (SE), and a 
novel shock capturing strategy without using a Riemann solver.  This method has been 
used to solve many types of flow problems, such as detonation waves, shock/acoustic 
wave interaction, cavitating flows, supersonic liquid jets, and chemically reacting flows.  In 
LS-DYNA, it has been extended to also solve fluid-structure interaction (FSI) problems.  It 
does this with two approaches.  The first approach solves the compressible flow equations 
on  an  Eulerian  mesh  while  the  structural  mechanics  is  solved  on  a  moving  mesh  that 
moves through the fixed CE/SE mesh.  In the second approach (new with this version), the 
CE/SE  mesh  moves  in  a  fashion  such  that  its  FSI  boundary  surface  matches  the 
corresponding  FSI  boundary  surface  of  the  moving  structural  mechanics  mesh.    This 
second approach is more accurate for FSI problems, especially with boundary layers flows.  
Another  new  feature  with  the  CESE  moving  mesh  solver  is  conjugate  heat  transfer 
coupling with the solid thermal solver.  The chemistry and stochastic particle solvers are 
two addon solvers that extend the CESE solver. 
The second solver is the incompressible flow solver (ICFD) that is fully coupled with the 
solid mechanics solver.  This coupling permits robust FSI analysis via either an explicit 
technique when the FSI is weak, or using an implicit coupling when the FSI coupling is
strong.  In addition to being able to handle free surface flows, there is also a bi-phasic flow 
capability  that  involves  modeling  using  a  conservative  Lagrangian  interface  tracking 
technique.  Basic turbulence models are also supported.  This solver is the first in LS-DYNA 
to make use of a new volume mesher that takes surface meshes bounding the fluid domain 
as  input  (*MESH  keywords).    In  addition,  during  the  time  advancement  of  the 
incompressible flow, the solution is adaptively re-meshed as an automatic feature of the 
solver.  Another important feature of the mesher is the ability to create boundary layer 
meshes.  These anisotropic meshes become a crucial part of the model when shear stresses 
are to be calculated near fluid walls.  The ICFD solver is also coupled to the solid thermal 
solver using a monolithic approach for conjugate heat transfer problems. 
The  third  solver  is  an  electromagnetics  (EM)  solver.    This  module  solves  the  Maxwell 
equations in the Eddy current (induction-diffusion) approximation.  This is suitable for 
cases where the propagation of electromagnetic waves in air (or vacuum) can be considered 
as instantaneous.  Therefore, the wave propagation is not solved.  The main applications 
are Magnetic Metal Forming, bending or welding, induced heating, ring expansions and so 
forth.  The EM module allows the introduction of a source of electrical current into solid 
conductors and the computation of the associated magnetic field, electric field, as well as 
induced  currents.    The  EM  solver  is coupled with the structural mechanics  solver (the 
Lorentz forces are added to the mechanics equations of motion), and with the structural 
thermal solver (the ohmic heating is added to the thermal solver as an extra source of heat).  
The EM fields are solved using a Finite Element Method (FEM) for the conductors and a 
Boundary Element Method (BEM) for the surrounding air/insulators.  Thus no air mesh is 
necessary. 
As stated above, the *CHEMISTRY and *STOCHASTIC cards are only used in the CESE 
solver at this time.
*CESE 
The keyword *CESE provides input data for the Conservation Element/Solution Element 
(CESE) compressible fluid solver: 
*CESE_BOUNDARY_AXISYMMETRIC_{OPTION} 
*CESE_BOUNDARY_BLAST_LOAD 
*CESE_BOUNDARY_CONJ_HEAT_{OPTION} 
*CESE_BOUNDARY_CYCLIC_{OPTION} 
*CESE_BOUNDARY_FSI_{OPTION} 
*CESE_BOUNDARY_NON_REFLECTIVE_{OPTION} 
*CESE_BOUNDARY_PRESCRIBED_{OPTION} 
*CESE_BOUNDARY_REFLECTIVE_{OPTION} 
*CESE_BOUNDARY_SLIDING_{OPTION} 
*CESE_BOUNDARY_SOLID_WALL_{OPTION1}_{OPTION2} 
*CESE_CHEMISTRY_D3PLOT 
*CESE_CONTROL_LIMITER 
*CESE_CONTROL_MESH_MOV 
*CESE_CONTROL_SOLVER 
*CESE_CONTROL_TIMESTEP 
*CESE_DATABASE_ELOUT 
*CESE_DATABASE_FLUXAVG 
*CESE_DATABASE_FSIDRAG 
*CESE_DATABASE_POINTOUT 
*CESE_DATABASE_SSETDRAG 
*CESE_DEFINE_NONINERTIAL 
*CESE_DEFINE_POINT
*CESE_EOS_CAV_HOMOG_EQUILIB 
*CESE 
*CESE_EOS_IDEAL_GAS 
*CESE_EOS_INFLATOR1 
*CESE_EOS_INFLATOR2 
*CESE_FSI_EXCLUDE 
*CESE_INITIAL 
*CESE_INITIAL_{OPTION} 
*CESE_INITIAL_CHEMISTRY 
*CESE_INITIAL_CHEMISTRY_ELEMENT 
*CESE_INITIAL_CHEMISTRY_PART 
*CESE_INITIAL_CHEMISTRY_SET 
*CESE_MAT_000 
*CESE_MAT_001 (*CESE_MAT_GAS) 
*CESE_MAT_002 
*CESE_PART 
*CESE_SURFACE_MECHSSID_D3PLOT 
*CESE_SURFACE_MECHVARS_D3PLOT 
Note that when performing a chemistry calculation with the CESE solver, initialization 
should only be done with the *CESE_INITIAL_CHEMISTRY_… cards, not the *CESE_INI-
TIAL… cards.
*CESE_BOUNDARY_AXISYMMETRIC_OPTION 
Available options are 
MSURF 
MSURF_SET 
SET 
SEGMENT 
Purpose: Define an axisymmetric boundary condition on the axisymmetric axis for the 2D 
axisymmetric CESE compressible flow solver.  
The MSURF and MSURF_SET options are used when the CESE mesh has been created 
using *MESH cards.  The SET and SEGMENT cards are used when *ELEMENT_SOLID 
cards are used to define the CESE mesh. 
Surface  Part  Card.  Card  1  format  used  when  the  MSURF  keyword  option  is  active. 
Provide as many cards as necessary.  This input ends at the next keyword (“*”) card. 
  Card 1a 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MSURFID 
Type 
I 
Default 
none 
Surface Part Set Card. Card 1 format used when the MSURF_SET keyword option is 
active.  Provide as many cards as necessary.  This input ends at the next keyword (“*”) 
card. 
  Card 1b 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MSURF_S 
Type 
I 
Default 
none
Set Card. Card 1 format used when the SET keyword option is active.  Provide as many 
cards as necessary.  This input ends at the next keyword (“*”) card. 
  Card 1c 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
Type 
I 
Default 
none 
Segment Cards. Card 1 format used when SEGMENT keyword option is active.  Include 
an additional card for each corresponding pair of segments.  This input ends at the next 
keyword (“*”) card. 
  Card 1d 
Variable 
1 
N1 
2 
N2 
3 
N3 
4 
N4 
5 
6 
7 
8 
Type 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
  VARIABLE   
MSURFID 
MSURF_S 
DESCRIPTION 
Mesh surface part ID referenced in *MESH_SURFACE_ELEMENT 
cards. 
Identifier of a set of mesh surface part IDs created with a *LSO_ID_-
SET card, where each mesh surface part ID in the set is referenced in
*MESH_SURFACE_ELEMENT cards. 
SSID 
Segment set ID 
N1, N2, … 
Node IDs defining a segment 
Remarks: 
1.  This boundary condition can only be used on the axisymmetric axis for the 2D 
axisymmetric CESE fluid solver.
*CESE_BOUNDARY_BLAST_LOAD_OPTION 
Available options include: 
MSURF 
MSURF_SET 
SET 
SEGMENT 
Purpose:  For the CESE compressible flow solver, set boundary values for velocity, density, 
and  pressure  from  a  blast  wave  defined  by  a  *LOAD_BLAST_ENHANCED  card.  
Boundary values are applied at the centroid of elements connected with this boundary.  
OPTION = SET  and  OPTION = SEGMENT  are  for  user  defined  meshes  whereas  OP-
TION = MSURF or MSURF_SET are associated with the automatic volume mesher .  
That is, the MSURF and MSURF_SET options are used when the CESE mesh has been 
created using *MESH cards.  The SET and SEGMENT cards are used when *ELEMENT_-
SOLID cards are used to define the CESE mesh. 
Surface Part Card. Card 1 format used when the MSURF keyword option is active. 
  Card 1a 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BID 
MSURFID 
Type 
I 
I 
Default 
none 
none 
Surface Part Set Card. Card 1 format used when the MSURF_SET keyword option is 
active. 
  Card 1b 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BID 
MSURF_S 
Type 
I 
I 
Default 
none 
none
Set Card. Card 1 format used when the SET keyword option is active. 
  Card 1c 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BID 
SSID 
Type 
I 
I 
Default 
none 
none 
Segment Card. Card 1 for SEGMENT keyword option is active. 
  Card 1d 
1 
Variable 
BID 
2 
N1 
3 
N2 
4 
N3 
5 
N4 
6 
7 
8 
Type 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
BID 
Blast source ID . 
MSURFID 
MSURF_S 
A mesh surface part ID referenced in *MESH_SURFACE_ELEMENT 
cards 
Identifier of a set of mesh surface part IDs created with a *LSO_ID_-
SET card, where each mesh surface part ID in the set is referenced in
*MESH_SURFACE_ELEMENT cards. 
SSID 
Segment set ID 
N1, N2, … 
Node ID’s defining a segment
*CESE_BOUNDARY_CONJ_HEAT_OPTION 
Available options are: 
MSURF 
MSURF_SET 
SET 
SEGMENT 
Purpose: Define a conjugate heat transfer interface condition for CESE compressible flows.  
This condition identifies those boundary faces of the CESE mesh that are in contact with 
non-moving structural parts, and through which heat flows.  This is only possible when the 
structural thermal solver is also in being used in the structural parts. 
The MSURF and MSURF_SET options are used when the CESE mesh has been created 
using *MESH cards.  The SET and SEGMENT cards are used when *ELEMENT_SOLID 
cards are used to define the CESE mesh. 
Surface Part Card.  Card 1 used when the MSURF keyword option is active.  Include  as 
many cards as necessary.  This input ends at the next keyword (“*”) card. 
  Card 1a 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MSURFID 
Type 
I 
Default 
none 
Surface Part Set Card.  Card 1 used when the MSURF_SET keyword option is active. 
Include  as many cards as necessary.  This input ends at the next keyword (“*”) card. 
  Card 1b 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MSURF_S 
Type 
I 
Default 
none
Set Card.  Card 1 used when the SET keyword option is active.  Include as many cards as 
necessary.  This input ends at the next keyword (“*”) card. 
  Card 1c 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
Type 
I 
Default 
none 
Segment Cards.  Card 1 used when SEGMENT keyword option is active.  Include an 
additional  card  for  each  corresponding  pair  of  segments.    This  input  ends  at  the  next 
keyword (“*”) card. 
  Card 1d 
Variable 
1 
N1 
2 
N2 
3 
N3 
4 
N4 
5 
6 
7 
8 
Type 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
  VARIABLE   
MSURFID 
MSURF_S 
DESCRIPTION 
Mesh surface part ID referenced in *MESH_SURFACE_ELEMENT 
cards. 
Identifier of a set of mesh surface part IDs created with an *LSO_-
ID_SET  card,  where  each  mesh  surface  part  ID  in  the  set  is 
referenced in *MESH_SURFACE_ELEMENT cards. 
SSID 
Segment set ID 
N1, N2, … 
Node IDs defining a segment 
Remarks: 
1.  This boundary condition should only be imposed on a CESE mesh boundary that 
is in contact with non-moving structural parts.  An Eulerian CESE solver is re-
quired, as is use of the structural thermal solver.
*CESE_BOUNDARY_CYCLIC_OPTION 
Available options are: 
MSURF 
MSURF_SET 
SET 
SEGMENT 
Purpose: Define a cyclic (periodic) boundary condition for CESE compressible flows.  This 
cyclic boundary condition (CBC) can be used on periodic boundary surfaces. 
The MSURF and MSURF_SET options are used when the CESE mesh has been created 
using *MESH cards.  The SET and SEGMENT cards are used when *ELEMENT_SOLID 
cards are used to define the CESE mesh. 
Card  Sets.    The  following  sequence  of  cards  comprises  a  single  set.    LS-DYNA  will 
continue reading *CESE_BOUNDARY_SOLID_WALL card sets until the next keyword 
(“*”) card is encountered. 
Surface Part Card. Card 1 format used when the MSURF keyword option is active. 
  Card 1a 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MSURFID1  MSURFID2  CYCTYP 
Type 
I 
I 
Default 
none 
none 
Remarks 
I 
0 
1, 2
Surface Part Set Card. Card 1 format used when the MSURF_SET keyword option is 
active. 
  Card 1b 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MSRF_S1  MSRF_S2  CYCTYP 
Type 
I 
I 
Default 
none 
none 
Remarks 
I 
0 
1, 3 
Set Card. Card 1 format used when the SET keyword option is active. 
  Card 1c 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID1 
SSID2 
CYCTYP 
Type 
I 
I 
Default 
none 
none 
Remarks 
I 
0 
1, 4 
Segment Card. Card 1 format used when SEGMENT keyword option is active.  Include an 
additional  card  for  each  corresponding  pair  of  segments.    This  input  ends  at  the  next 
keyword (“*”) card. 
  Card 1d 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ND1 
ND2 
ND3 
ND4 
NP1 
NP2 
NP3 
NP4 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none
Rotation  Case  Card.  Additional  card  for  the  MSURF,  MSURF_SET,  and  SET  options 
when CYCTYP = 1. 
  Card 2a 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
AXISX1 
AXISY1 
AXISZ1 
DIRX 
DIRY 
DIRZ 
ROTANG 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
none 
none 
none 
none 
Translation Case Card. Additional card for the MSURF, MSURF_SET, and SET options 
when CYCTYP = 2. 
  Card 2b 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TRANSX 
TRANSY 
TRANSZ 
Type 
F 
F 
F 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION
MSURFID1, 
MSURFID2 
Mesh surface part numbers referenced in *MESH_SURFACE_ELE-
MENT cards. 
MSRF_S1, 
MSRF_S2 
Identifiers of two sets of mesh surface part IDs, each created with
a *LSO_ID_SET card, where each mesh surface part ID in each set 
is referenced in *MESH_SURFACE_ELEMENT cards. 
CYCTYP 
Relationship between the two cyclic boundary condition surfaces:
EQ.0: none assumed (default) 
EQ.1: The  first  surface  is  rotated  about  an  axis  to  match  the
second surface. 
EQ.2: The  faces  of  the  first  surface  are  translated  in  a  given
direction to obtain the corresponding faces on the second
surface. 
SSID1 & SSID2 
A pair of segment set IDs
*CESE_BOUNDARY_CYCLIC 
Node  IDs  defining  a  pair  of  segments:  ND1,  ND2,  ND3,  ND4
define the first segment, while NP1, NP2, NP3, NP4 define the
second segment.  This pair of segments must match either through
a geometric translation or rotation. 
AXIS[Z,Y,Z]1 
A point on the axis of rotation for CYCTYP.EQ.1. 
DIR[X,Y,Z] 
ROTANG 
The direction which together with AXIS[X,Y,Z]1 defines the axis
of rotation for CYCTYP.EQ.1. 
The angle of rotation (in degrees) that transforms the centroid of
each face on the first surface to the centroid of the corresponding 
face on the second surface (for CYCTYP.EQ.1). 
TRANS[X,Y,Z] 
The  translation  direction  that  enables  the  identification  of  the
segment in the second surface that matches a segment in the first
surface (for CYCTYP.EQ.2). 
Remarks: 
1.  For  the  MSURF,  MSURF_SET,  or  SET  options  with  CYCTYP.EQ.0,  the  code 
examines the geometry of two faces of the two surfaces in order to determine if the 
surfaces are approximately parallel (CYCTYP.EQ.2), or related through a rotation 
(CYCTYP.EQ.1).  The geometric parameters required are then computed. 
2.  For the MSURF option, there must be the same number of mesh surface elements 
in each mesh surface part, and the mesh surface elements in each mesh surface 
part are then internally ordered in order to match pairwise between the two mesh 
surface parts. 
3.  For  the  MSURF_SET  option,  there  must  be  the  same  number  of  mesh  surface 
elements in each mesh surface part set, and the mesh surface elements in each 
mesh surface part set are then internally ordered in order to match pairwise be-
tween the two mesh surface part sets. 
4.  For the SET option, there must be the same number of segments in each set, and 
the segments in each set are then internally ordered in order to match pairwise 
between the two sets.
*CESE_BOUNDARY_FSI_OPTION 
Available options are: 
MSURF 
MSURF_SET 
SET 
SEGMENT 
Purpose: Define an FSI boundary condition for the moving mesh CESE compressible flow 
solver.    This  card  must  not  be  combined  with  the  immersed-boundary  method  CESE 
solver, and doing so will result in an error termination condition. 
This boundary condition must be applied on a surface of the CESE computational domain 
that is co-located with surfaces of the outside boundary of the structural mechanics mesh.  
The nodes of the two meshes will generally not be shared. 
The MSURF and MSURF_SET options are used when the CESE mesh has been created 
using *MESH cards.  The SET and SEGMENT cards are used when *ELEMENT_SOLID 
cards are used to define the CESE mesh. 
Surface  Part  Card.  Card  1  format  used  when  the  MSURF  keyword  option  is  active. 
Provide as many cards as necessary.  This input ends at the next keyword (“*”) card. 
  Card 1a 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MSURFID 
Type 
I 
Default 
none
Surface Part Set Card. Card 1 format used when the MSURF_SET keyword option is 
active.  Provide as many cards as necessary.  This input ends at the next keyword (“*”) 
card. 
  Card 1b 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MSURF_S 
Type 
I 
Default 
none 
Set Card. Card 1 format used when the SET keyword option is active.  Provide as many 
cards as necessary.  This input ends at the next keyword (“*”) card. 
  Card 1c 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
Type 
I 
Default 
none 
Segment Cards. Card 1 format used when SEGMENT keyword option is active.  Include 
an additional card for each corresponding pair of segments.  This input ends at the next 
keyword (“*”) card. 
  Card 1d 
Variable 
1 
N1 
2 
N2 
3 
N3 
4 
N4 
5 
6 
7 
8 
Type 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
  VARIABLE   
MSURFID 
DESCRIPTION 
Mesh surface part ID referenced in *MESH_SURFACE_ELEMENT 
cards.
VARIABLE   
MSURF_S 
DESCRIPTION 
Identifier of a set of mesh surface part IDs created with a *LSO_ID_-
SET card, where each mesh surface part ID in the set is referenced in 
*MESH_SURFACE_ELEMENT cards. 
SSID 
Segment set ID. 
N1, … 
Node IDs defining a segment 
Remarks: 
1.  This boundary condition card is also needed for conjugate heat transfer problems 
with the moving mesh CESE solver.
*CESE_BOUNDARY_NON_REFLECTIVE_OPTION 
Available options are: 
MSURF 
MSURF_SET 
SET 
SEGMENT 
Purpose: Define a passive boundary condition for CESE compressible flows.  This non-
reflective boundary condition (NBC) provides an artificial computational boundary for an 
open boundary that is passive. 
The MSURF and MSURF_SET options are used when the CESE mesh has been created 
using *MESH cards.  The SET and SEGMENT cards are used when *ELEMENT_SOLID 
cards are used to define the CESE mesh. 
Surface Part Card.  Card 1 used when the MSURF keyword option is active.  Include  as 
many cards as necessary.  This input ends at the next keyword (“*”) card. 
  Card 1a 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MSURFID 
Type 
I 
Default 
none 
Surface Part Set Card.  Card 1 used when the MSURF_SET keyword option is active. 
Include  as many cards as necessary.  This input ends at the next keyword (“*”) card. 
  Card 1b 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MSURF_S 
Type 
I 
Default 
none
Set Card.  Card 1 used when the SET keyword option is active.  Include as many cards as 
necessary.  This input ends at the next keyword (“*”) card. 
  Card 1c 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
Type 
I 
Default 
none 
Segment Cards.  Card 1 used when SEGMENT keyword option is active.  Include an 
additional  card  for  each  corresponding  pair  of  segments.    This  input  ends  at  the  next 
keyword (“*”) card. 
  Card 1d 
Variable 
1 
N1 
2 
N2 
3 
N3 
4 
N4 
5 
6 
7 
8 
Type 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
  VARIABLE   
MSURFID 
MSURF_S 
DESCRIPTION 
Mesh surface part ID referenced in *MESH_SURFACE_ELEMENT 
cards. 
Identifier of a set of mesh surface part IDs created with an *LSO_-
ID_SET  card,  where  each  mesh  surface  part  ID  in  the  set  is 
referenced in *MESH_SURFACE_ELEMENT cards. 
SSID 
Segment set ID 
N1, N2, … 
Node IDs defining a segment 
Remarks: 
1.  This boundary condition is usually imposed on an open surface that is far from the 
main disturbed flow (the further away, the better), i.e., the flow on that boundary 
surface should be almost uniform.
2. 
If any boundary segment has not been assigned a boundary condition by any of 
the *CESE_BOUNDARY_… cards, then it will automatically be assigned this non-
reflective boundary condition.
*CESE_BOUNDARY_PRESCRIBED_OPTION 
Available options include: 
MSURF 
MSURF_SET 
SET 
SEGMENT 
Purpose:  For the CESE compressible flow solver, set boundary values for velocity, density, 
pressure  and  temperature.    Boundary  values  are  applied  at  the  centroid  of  elements 
connected with this boundary.  OPTION = SET and OPTION = SEGMENT are for user 
defined  meshes  whereas  OPTION = MSURF  or  MSURF_SET  are  associated  with  the 
automatic volume mesher .  
That is, the MSURF and MSURF_SET options are used when the CESE mesh has been 
created  using  *MESH  cards. 
  The  SET  and  SEGMENT  cards  are  used  when 
*ELEMENT_SOLID cards are used to define the CESE mesh. 
Card Sets: 
A set of data cards for this keyword consists of 3 of the following cards: 
1.  Card 1 specifies the object to which the boundary condition is applied.  Its format 
depends on the keyword option. 
2.  Card 2 reads in load curve IDs. 
3.  Card 3 reads in scale factors. 
For each boundary condition to be specified include one set of cards.  This input ends at the 
next keyword (“*”) card. 
Surface Part Card. Card 1 format used when the MSURF keyword option is active. 
  Card 1a 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MSURFID 
IDCOMP 
Type 
I 
I 
Default 
none 
none
Surface Part Set Card. Card 1 format used when the MSURF_SET keyword option is 
active. 
  Card 1b 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MSURF_S 
IDCOMP 
Type 
I 
I 
Default 
none 
none 
Set Card. Card 1 format used when the SET keyword option is active. 
  Card 1c 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
IDCOMP 
Type 
I 
I 
Default 
none 
none 
Segment Card. Card 1 for SEGMENT keyword option is active. 
  Card 1d 
Variable 
1 
N1 
2 
N1 
3 
N3 
4 
N4 
5 
6 
7 
8 
IDCOMP 
Type 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none
Load Curve Card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LC_U 
LC_V 
LC_W 
LC_RHO 
LC_P 
LC_T 
Type 
I 
I 
I 
I 
I 
I 
Remarks 
1,2,3 
1,2,3 
1,2,3 
1,2,3 
1,2,3 
1,2,3 
Scale Factor Card. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SF_U 
SF_V 
SF_W 
SF_RHO 
SF_P 
SF_T 
Type 
F 
F 
F 
F 
F 
F 
Default 
1.0 
1.0 
1.0 
1.0 
1.0 
1.0 
Remarks 
2 
2 
2 
2 
2 
2 
  VARIABLE   
MSURFID 
MSURF_S 
DESCRIPTION 
A mesh surface part ID referenced in *MESH_SURFACE_ELEMENT 
cards 
Identifier of a set of mesh surface part IDs created with a *LSO_ID_-
SET card, where each mesh surface part ID in the set is referenced in
*MESH_SURFACE_ELEMENT cards. 
SSID 
Segment set ID 
N1, N2, … 
Node ID’s defining a segment 
IDCOMP 
For  inflow  boundaries  in  problems  involving  chemical  reacting
flows,  the  chemical  mixture  of  the  fluid  entering  the  domain  is
defined with a *CHEMISTRY_COMPOSITION card with this ID. 
LC_U 
Load curve ID to describe the x-component of the velocity versus 
time; see *DEFINE_CURVE.
LC_V 
LC_W 
*CESE_BOUNDARY_PRESCRIBED 
DESCRIPTION 
Load curve ID to describe the y-component of the velocity versus 
time. 
Load curve ID to describe the z-component of the velocity versus 
time. 
LC_RHO 
Load curve ID to describe the density versus time. 
LC_P 
LC_T 
SF_U 
SF_V 
Load curve ID to describe the pressure versus time. 
Load curve ID to describe the temperature versus time. 
Scale factor for LC_U (default = 1.0). 
Scale factor for LC_V (default = 1.0). 
SF_W 
Scale factor for LC_W (default = 1.0). 
SF_RHO 
Scale factor for LC_RHO (default = 1.0). 
Scale factor for LC_P (default = 1.0). 
Scale factor for LC_T (default = 1.0). 
SF_P 
SF_T 
Remarks: 
1.  On each centroid or set of centroids, the variables (𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝜌, 𝑃, 𝑇) that are given 
values must be consistent and make the model well-posed (i.e., be such that the 
solution of the model exists, is unique and physical). 
2. 
3. 
If any of the load curves are 0, the corresponding variable will take the constant 
value of the corresponding scale factor.  For instance, if LC_RHO = 0, then the 
constant value of the density for this boundary condition will be SF_RHO. 
If a load ID is -1 for a given variable, then the boundary value for that variable is 
computed by the solver, and not specified by the user.
*CESE_BOUNDARY_REFLECTIVE_OPTION 
Available options are: 
MSURF 
MSURF_SET 
SET 
SEGMENT 
Purpose: Define a reflective boundary condition (RBC) for the CESE compressible flow 
solver.  This boundary condition can be applied on a symmetrical surface or a solid wall of 
the computational domain. 
The MSURF and MSURF_SET options are used when the CESE mesh has been created 
using *MESH cards.  The SET and SEGMENT cards are used when *ELEMENT_SOLID 
cards are used to define the CESE mesh. 
Surface  Part  Card.  Card  1  format  used  when  the  MSURF  keyword  option  is  active. 
Provide as many cards as necessary.  This input ends at the next keyword (“*”) card. 
  Card 1a 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MSURFID 
Type 
I 
Default 
none 
Surface Part Set Card. Card 1 format used when the MSURF_SET keyword option is 
active.  Provide as many cards as necessary.  This input ends at the next keyword (“*”) 
card. 
  Card 1b 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MSURF_S 
Type 
I 
Default 
none
Set Card. Card 1 format used when the SET keyword option is active.  Provide as many 
cards as necessary.  This input ends at the next keyword (“*”) card. 
  Card 1c 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
Type 
I 
Default 
none 
Segment Cards. Card 1 format used when SEGMENT keyword option is active.  Include 
an additional card for each corresponding pair of segments.  This input ends at the next 
keyword (“*”) card. 
  Card 1d 
Variable 
1 
N1 
2 
N2 
3 
N3 
4 
N4 
5 
6 
7 
8 
Type 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
  VARIABLE   
MSURFID 
MSURF_S 
DESCRIPTION 
Mesh surface part ID referenced in *MESH_SURFACE_ELEMENT 
cards. 
Identifier of a set of mesh surface part IDs created with a *LSO_ID_-
SET card, where each mesh surface part ID in the set is referenced in 
*MESH_SURFACE_ELEMENT cards. 
SSID 
Segment set ID. 
N1, N2, … 
Node IDs defining a segment 
Remarks: 
1.  This boundary condition has the same effect as a solid-wall boundary condition for 
inviscid flows.
*CESE_BOUNDARY_SLIDING_OPTION 
Available options are: 
MSURF 
MSURF_SET 
SET 
SEGMENT 
Purpose:  Allows  nodes  of  a  fluid  surface  to  translate  in  the  main  direction  of  mesh 
movement.  This is useful in piston type applications.  
The MSURF and MSURF_SET options are used when the CESE mesh has been created 
using *MESH cards.  The SET and SEGMENT cards are used when *ELEMENT_SOLID 
cards are used to define the CESE mesh. 
Surface  Part  Card.  Card  1  format  used  when  the  MSURF  keyword  option  is  active. 
Provide as many cards as necessary.  This input ends at the next keyword (“*”) card. 
  Card 1a 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MSURFID 
Type 
I 
Default 
none 
Surface Part Set Card. Card 1 format used when the MSURF_SET keyword option is 
active.  Provide as many cards as necessary.  This input ends at the next keyword (“*”) 
card. 
  Card 1b 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MSURF_S 
Type 
I 
Default 
none
Set Card. Card 1 format used when the SET keyword option is active.  Provide as many 
cards as necessary.  This input ends at the next keyword (“*”) card. 
  Card 1c 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
Type 
I 
Default 
none 
Segment Cards. Card 1 format used when SEGMENT keyword option is active.  Include 
an additional card for each corresponding pair of segments.  This input ends at the next 
keyword (“*”) card. 
  Card 1d 
Variable 
1 
N1 
2 
N2 
3 
N3 
4 
N4 
5 
6 
7 
8 
Type 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
  VARIABLE   
MSURFID 
MSURF_S 
DESCRIPTION 
Mesh surface part ID referenced in *MESH_SURFACE_ELEMENT 
cards. 
Identifier of a set of mesh surface part IDs created with a *LSO_ID_-
SET card, where each mesh surface part ID in the set is referenced in
*MESH_SURFACE_ELEMENT cards. 
SSID 
Segment set ID 
N1, N2, … 
Node IDs defining a segment
*CESE_BOUNDARY_SOLID_WALL_OPTION1_OPTION2 
For OPTION1 the choices are: 
MSURF 
MSURF_SET 
SET 
SEGMENT 
For OPTION2 the choices are: 
<BLANK> 
ROTAT 
Purpose: Define a solid wall boundary condition (SBC) for this CESE compressible flow 
solver.  This boundary condition can be applied at a solid boundary that is the physical 
boundary for the flow field.  For inviscid flow, this will be a slip boundary condition; while 
for viscous flows, it is a no-slip boundary condition. 
The MSURF and MSURF_SET options are used when the CESE mesh has been created 
using *MESH cards.  The SET and SEGMENT cards are used when *ELEMENT_SOLID 
cards are used to define the CESE mesh. 
Card  Sets.    The  following  sequence  of  cards  comprises  a  single  set.    LS-DYNA  will 
continue reading *CESE_BOUNDARY_SOLID_WALL card sets until the next keyword 
(“*”) card is encountered. 
Surface Part Card.  Card 1 format used when the MSURF keyword option is active.  
  Card 1a 
1 
2 
Variable  MSURFID 
LCID 
Type 
I 
Default 
none 
I 
0 
3 
Vx 
F 
4 
Vy 
F 
5 
Vz 
F 
6 
Nx 
F 
7 
Ny 
F 
8 
Nz 
F 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Remarks 
2, 3 
2 
2 
2 
3 
3
Surface Part Set Card.  Card 1 format used when the MSURF_SET keyword option is 
active.  
  Card 1b 
1 
2 
Variable  MSURF_S 
LCID 
Type 
I 
Default 
none 
I 
0 
3 
Vx 
F 
4 
Vy 
F 
5 
Vz 
F 
6 
Nx 
F 
7 
Ny 
F 
8 
Nz 
F 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Remarks 
2, 3 
2 
2 
2 
3 
3 
3 
Set Card. Card 1 format used when the SET keyword option is active.  
  Card 1c 
1 
2 
Variable 
SSID 
LCID 
Type 
I 
Default 
none 
I 
0 
3 
Vx 
F 
4 
Vy 
F 
5 
Vz 
F 
6 
Nx 
F 
7 
Ny 
F 
8 
Nz 
F 
0.0 
0.0 
0.0 
0.0 
0.0 
0.0 
Remarks 
2, 3 
2 
2 
2 
3 
3 
3 
Segment Card. Card 1 format used when SEGMENT keyword option is active. 
  Card 1d 
Variable 
1 
N1 
2 
N2 
3 
N3 
4 
N4 
5 
LCID 
Type 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
I 
0 
6 
Vx 
F 
7 
Vy 
F 
8 
Vz 
F 
0.0 
0.0 
0.0 
Remarks 
2, 3 
2 
2
Rotating Axis Card.  Additional card read when the ROTAT keyword option is set. 
4 
5 
6 
7 
8 
  Card 2 
Variable 
1 
Nx 
Type 
F 
2 
Ny 
F 
3 
Nz 
F 
Default 
0.0 
0.0 
0.0 
Remarks 
3 
3 
3 
  VARIABLE   
MSURFID 
MSURF_S 
DESCRIPTION 
Mesh surface part ID referenced in *MESH_SURFACE_ELEMENT 
cards. 
Identifier of a set of mesh surface part IDs created with a *LSO_ID_-
SET card, where each mesh surface part ID in the set is referenced in
*MESH_SURFACE_ELEMENT cards. 
SSID 
Segment set ID 
N1, N2, … 
Node ID’s defining a segment 
LCID 
Load curve ID to define this solid wall boundary movement 
If OPTION2 = <BLANK>: 
Vx, Vy, Vz 
velocity vector of the solid wall: 
LCID.EQ.0: it is defined by (Vx, Vy, Vz) itself; 
LCID.NE.0:  it  will  be  defined  by  both  of  the  load  curve  and
(Vx, Vy, Vz); Nx, Ny, Nz are not used in this case. 
If OPTION2 = ROTAT: 
Vx, Vy, Vz 
x-,y- & z-coordinates of a point on the rotating axis 
Nx, Ny, Nz 
Unit vector of the rotating axis (for the 2D case, this is not used). 
The rotating frequency (Hz) is given by the load curve.
*CESE_BOUNDARY_SOLID_WALL 
1. 
In  this  solid-wall  condition  (SBC),  the  boundary  movement  can  only  be  in  the 
tangential direction of the wall and should not affect the fluid domain size and 
mesh during the calculation, otherwise an FSI or moving mesh solver should be 
used.  Also, this moving SBC only affects viscous flows (no-slip BC). 
2. 
If LCID = 0 and Vx = Vy = Vz = 0.0 (default), this will be a regular solid wall BC. 
3.  For rotating SBC, LCID > 0 must be used to define the rotating speed frequency 
(Hz).  Also, in the 2D case, (Nx, Ny, Nz) does not need to be defined because it is 
not needed.
*CESE 
Purpose:  Cause  mass  fractions of the listed  chemical species to be added to the CESE 
d3plot output.  This is only used when chemistry is being solved with the CESE solver. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MODELID 
Type 
I 
Default 
none 
Species Cards.  Include one card for each species to be included in the d3plot database. 
This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
SPECIES 
A 
  VARIABLE   
DESCRIPTION 
MODELID 
Identifier of a Chemkin-compatible chemistry model. 
SPECIES 
Name of a chemical species that is defined in the chemistry model
identified by MODELID .
*CESE_CONTROL_LIMITER 
Purpose:  Sets  some  stability  parameters  used  in  the  CESE  scheme  for  this  CESE 
compressible flow solver. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IDLMT 
ALFA 
BETA 
EPSR 
Type 
Default 
I 
0 
F 
F 
F 
0.0 
0.0 
0.0 
Remarks 
1 
2 
3 
  VARIABLE   
DESCRIPTION 
IDLMT 
Set the stability limiter option : 
EQ.0: limiter format 1 (Re-weighting). 
EQ.1: limiter format 2 (Relaxing). 
Re-weighting coefficient  
Numerical viscosity control coefficient 
Stability control coefficient  
ALFA 
BETA 
EPSR 
Remarks: 
1.  𝛼 ≥ 0; larger values give more stability, but less accuracy.  Usually α = 2.0 or 4.0 
will be enough for normal shock problems. 
2. 
3. 
0 ≤ 𝛽 ≤ 1;  larger  values  give  more  stability.    For  problems  with  shock  waves, 
β = 1.0 is recommended. 
𝜀 ≥ 0; larger values give more stability, but less accuracy.
*CESE 
Purpose:  For moving mesh CESE, this keyword is used to choose the type of algorithm to 
be used for calculating mesh movement. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MMSH 
LIM_ITER  RELTOL 
Type 
Default 
I 
1 
I 
F 
100 
1.0e-3 
  VARIABLE   
DESCRIPTION 
MMSH 
Mesh motion selector: 
EQ.1: mesh moves using an implicit ball-vertex spring method.
EQ.9: the IDW scheme is used to move the mesh. 
Maximum number of linear solver iterations for the implicit ball-
vertex spring linear system. 
Relative  tolerance  to  use  as  a  stopping  criterion  for  the  iterative
linear  solver  (conjugate  gradient  solver  with  diagonal  scaling
preconditioner). 
LIM_ITER 
RELTOL 
.
*CESE_CONTROL_SOLVER 
Purpose:  Set general purpose control variables for the CESE compressible flow solver. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ICESE 
IFLOW 
IGEOM 
IFRAME 
MIXID 
IDC 
ISNAN 
Type 
Default 
I 
0 
I 
0 
Remarks 
I 
none 
1, 2 
I 
0 
I 
F 
none 
0.25 
I 
0 
3 
  VARIABLE   
DESCRIPTION 
ICESE 
Sets the framework of the CESE solver. 
EQ.0: 
Fixed Eulerian 
EQ.100:  Moving Mesh FSI 
EQ.200:  Immersed boundary FSI 
IFLOW 
Sets the compressible flow types: 
EQ.0: Viscous flows (laminar) 
EQ.1: Invisid flows 
IGEOM 
Sets the geometric dimension: 
EQ.2:  Two-dimensional (2D) problem 
EQ.3:  Three-dimensional (3D) problem 
EQ.101:  2D axisymmetric 
IFRAME 
Choose the frame of reference: 
EQ.0: 
Usual non-moving reference frame (default). 
EQ.1000:  Non-inertial rotating reference frame. 
MIXID 
Chemistry model ID that defines the chemical species to include in
the  mixing  model  .    The  species 
information  is  given  through  the  model’s  card  specifying  the
Chemkin-compatible input.
VARIABLE   
DESCRIPTION 
Contact interaction detection coefficient (for FSI and conjugate heat 
transfer problems). 
Flag to check for a NaN in the CESE solver solution arrays at the
completion  of  each  time  step.    This  option  can  be  useful  for
debugging purposes.  There is a cost overhead when this option is
active. 
EQ.0: No checking, 
EQ.1: Checking is active. 
IDC 
ISNAN 
Remarks: 
1. 
If the user wants to use the 2D (IGEOM = 2) or 2D axisymmetric (IGEOM = 101) 
solver, the mesh should only be distributed in the x-y plane with the boundary 
conditions given only at the 𝑥-𝑦 domain boundaries.  Otherwise, a warning mes-
sage will be given and the 3D solver will be triggered instead. 
2.  The  2D  axisymmetric  case  will  work  only  if  the  2D  mesh  and  corresponding 
boundary conditions are properly defined, with the 𝑥 and 𝑦 coordinates corre-
sponding to the radial and axial directions respectively. 
3. 
IDC is the same type of variable that is input on the *ICFD_CONTROL_FSI card.  
For an explanation, see Remark 1 for the *ICFD_CONTROL_FSI card.
*CESE_CONTROL_TIMESTEP 
Purpose:  Sets the time-step control parameters for the CESE compressible flow solver.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IDDT 
CFL 
DTINT 
Type 
Default 
I 
0 
F 
F 
0.9 
1.0E-3 
  VARIABLE   
DESCRIPTION 
IDDT 
Sets the time step option: 
EQ.0: Fixed  time  step  size  (DTINT,  i.e.,  given  initial  time  step
size) 
NE.0:  the  time  step  size  will  be  calculated  based  on  the  given 
CFL-number  and  the  flow  solution  at  the  previous  time
step. 
CFL 
CFL number (Courant–Friedrichs–Lewy condition) 
( 0.0 < CFL ≤ 1.0 ) 
DTINT 
Initial time step size
*CESE 
Purpose:  This keyword enables the output of CESE data on elements.  If more than one 
element set is defined, then several output files will be generated. 
Output Options Card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OUTLV 
DTOUT 
Type 
Default 
I 
0 
F 
0. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ELSID 
Type 
I 
Default 
none 
  VARIABLE   
DESCRIPTION 
OUTLV 
Determines if the output file should be dumped. 
EQ.0:  No output file is generated. 
EQ.1:  The output file is generated. 
DTOUT 
Time interval to print the output.  If DTOUT is equal to 0.0, then the
CESE timestep will be used. 
ELSID 
Solid Elements Set ID. 
Remarks: 
1.  The file name for this database is cese_elout.dat.
*CESE_CONTROL_TIMESTEP 
Purpose:  This keyword enables the output of CESE data on segment sets.  If more than one 
segment set is defined, then several output files will be generated. 
Output Options Card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OUTLV 
DTOUT 
Type 
Default 
I 
0 
F 
0. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
Type 
I 
Default 
none 
  VARIABLE   
DESCRIPTION 
OUTLV 
Determines if the output file should be dumped. 
EQ.0:  No output file is generated. 
EQ.1:  The output file giving the average fluxes is generated. 
DTOUT 
Time interval to print the output.  If DTOUT is equal to 0.0, then the
CESE timestep will be used. 
SSID 
Segment Set ID. 
Remarks: 
1.  The file names for this database is cese_fluxavg.dat.
*CESE 
Purpose:  This keyword enables the output of the total fluid pressure force applied on solid 
parts in FSI problems at every time step. 
Output Options Card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OUTLV 
Type 
Default 
I 
0 
  VARIABLE   
DESCRIPTION 
OUTLV 
Determines if the output file should be dumped. 
EQ.0:  No output file is generated. 
EQ.1:  The output file giving the pressure forces is generated. 
Remarks: 
1.  The  file  names  for  this  database  are  cese_dragsol.dat,  cese_dragshell.dat, 
cese_dragsol2D.dat and cese_dragbeam.dat .depending on what kind of solid is 
used.
*CESE_CONTROL_TIMESTEP 
Purpose:  This keyword enables the output of CESE data on points. 
Output Options Card. 
  Card 1 
1 
2 
3 
Variable 
PSID 
DTOUT 
PSTYPE 
Type 
Default 
I 
0 
F 
0. 
I 
0 
4 
VX 
F 
0. 
5 
VY 
F 
0. 
6 
VZ 
F 
0. 
7 
8 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
5 
6 
7 
8 
  Card 2 
1 
Variable 
PID 
Type 
I 
2 
X 
F 
3 
Y 
F 
4 
Z 
F 
Default 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
PSID 
Point Set ID. 
DTOUT 
Time interval to print the output.  If DTOUT is equal to 0.0, then the
CESE timestep will be used. 
PSTYPE 
Point Set type : 
EQ.0: Fixed points. 
EQ.1: Tracer points using prescribed velocity. 
EQ.2:  Tracer points using fluid velocity. 
VX, VY, VZ 
Constant velocities to be used when PSTYPE = 1 
PID 
Point ID 
X, Y, Z 
Point initial coordinates
Remarks: 
1.  The file name for this database is cese_pointout.dat.
*CESE_DATABASE_SSETDRAG 
Purpose:  This keyword enables the output of CESE drag forces on segment sets.  If more 
than one segment set is defined, then several output files will be generated. 
Output Options Card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OUTLV 
DTOUT 
Type 
Default 
I 
0 
F 
0. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
Type 
I 
Default 
none 
  VARIABLE   
DESCRIPTION 
OUTLV 
Determines if the output file should be dumped. 
EQ.0:  No output file is generated. 
EQ.1:  The output file giving the average fluxes is generated. 
DTOUT 
Time interval to print the output.  If DTOUT is equal to 0.0, then the
CESE timestep will be used. 
SSID 
Segment Set ID. 
Remarks: 
1.  The file name for this database is cese_ssetdrag.dat.
2. 
In order for the friction drag to give consistent results, special care must be given 
to the mesh close to the solid wall boundary (Good capturing of the boundary 
layer behavior).  A very fine structured mesh is recommended.
*CESE_DEFINE_NONINERTIAL 
Purpose: Define the CESE problem domain as a non-inertial rotating frame that rotates at a 
constant rate.  This is used in rotating problems such as spinning cylinders, wind turbines 
and turbo machinery. 
  Card 1 
1 
2 
Variable 
FREQ 
LCID 
Type 
F 
Default 
none 
  Card 2 
Variable 
Type 
1 
L 
F 
I 
0 
2 
R 
F 
Default 
none 
none 
7 
8 
3 
PID 
I 
4 
Nx 
F 
5 
Ny 
F 
6 
Nz 
F 
none 
none 
none 
none 
3 
4 
5 
6 
7 
8 
RELV 
I 
0 
  VARIABLE   
DESCRIPTION 
FREQ 
LCID 
PID 
Frequency of rotation. 
Load curve ID for scaling factor of FREQ. 
Starting  point  ID  for  the  reference  frame  . 
Nx, Ny, Nz 
Rotating axis direction. 
L 
R 
Length of rotating frame. 
Radius of rotating frame.
VARIABLE   
DESCRIPTION 
RELV 
Velocity display mode: 
EQ.0:  Relative velocity, only the non-rotating components of the 
velocity are output. 
EQ.1:  Absolute velocity is output.
*CESE_POINT 
Purpose: Define points to be used by the CESE solver. 
Point Cards.  Include one card for each point.  This input ends at the next keyword (“*”) 
card. 
5 
6 
7 
8 
  Card 1 
1 
Variable 
NID 
Type 
I 
2 
X 
F 
3 
Y 
F 
4 
Z 
F 
Default 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
NID 
Identifier for this point. 
X, Y, Z 
Coordinates of the point.
*CESE 
Purpose:  Provide the far-field (or free-stream) fluid pressure. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PRESS 
Type 
F 
  VARIABLE   
PRESS 
DESCRIPTION 
Value of the free-stream fluid pressure (in units used by the current 
problem).
*CESE_EOS_CAV_HOMOG_EQUILIB 
Purpose:  Define  the  coefficients  in  the  equation  of  state  (EOS)  for  the  homogeneous 
equilibrium cavitation model. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
Variable 
EOSID 
2 
vap 
3 
liq 
4 
𝑎vap 
5 
𝑎liq 
6 
vap 
7 
liq 
8 
𝑃SatVap 
Type 
I 
F 
F 
F 
F 
F 
F 
Default 
none 
0.8 
880.0 
334.0 
1386.0 
1.435e-
5 
1.586e-
4 
1.2e+4 
  VARIABLE   
DESCRIPTION 
EOSID 
Equation of state identifier 
vap 
liq 
𝑎vap 
𝑎liq 
vap 
liq 
density of the saturated vapor 
density of the saturated liquid 
sound speed of the saturated vapor 
sound speed of the saturated liquid 
dynamic viscosity of the vapor 
dynamic viscosity of the liquid 
𝑃SatVap 
pressure of the saturated vapor 
Remarks: 
1.  Once a cavitation EOS is used, the cavitation flow solver will be triggered. 
2. 
In this homogeneous equilibrium cavitation model, a barotropic equation of state 
is used.  This model can be used in small scale & high speed cavitation flows, and 
it is not good for large-scale, low-speed cavitation calculations.
*CESE 
Purpose: Define the coefficients Cv and Cp in the equation of state for an ideal gas in the 
CESE fluid solver. 
4 
5 
6 
7 
8 
  Card 1 
1 
Variable 
EOSID 
Type 
I 
2 
Cv 
F 
3 
Cp 
F 
Default 
none 
717.5 
1004.5 
  VARIABLE   
DESCRIPTION 
EOSID 
Equation of state identifier 
Cv 
Cp 
Specific heat at constant volume 
Specific heat at constant pressure 
Remarks: 
1.  As with other solvers in LS-DYNA, the user is responsible for unit consistency.  
For example, if a user wants to use dimensionless variables, Cv & Cp above also 
should be replaced by the corresponding dimensionless ones.
*CESE_EOS_INFLATOR1 
Purpose:  To define an EOS using Cp and Cv thermodynamic expansions for an inflator gas 
mixture with a single temperature range. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EOSID 
Type 
I 
Default 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Cp0 
Cp1 
Cp2 
Cp3 
Cp4 
Type 
F 
Default 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Cv0 
Cv1 
Cv2 
Cv3 
Cv4 
Type 
F 
Default 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
  VARIABLE   
DESCRIPTION 
EOSID 
Equation of state identifier for the CESE solver. 
Cp0, …, Cp4 
Coefficients  of  temperature-dependent  specific  heat  at  constant 
pressure 
Cp(T) = Cp0 + Cp1 T + Cp2 T2 + Cp3 T3 + Cp4 T4
DESCRIPTION 
Coefficients  of  temperature-dependent  specific  heat  at  constant 
volume 
Cv(T) = Cv0 + Cv1 T + Cv2 T2 + Cv3 T3 + Cv4 T4 
  VARIABLE   
Cv0, …, Cv4 
Remark: 
1.These coefficient expansions for the specific heats over the entire temperature range 
are 
See 
and 
*CHEMISTRY_CONTROL_INFLATOR 
*CHEMISTRY_INFLATOR_PROPERTIES for details related to running that solver.
inflator  model 
generated 
solver. 
0-D 
the 
by
*CESE_EOS_INFLATOR2 
Purpose:  To define an EOS using Cp and Cv thermodynamic expansions for an inflator gas 
mixture with two temperature ranges, one below 1000 degrees Kelvin, and the other above 
1000 degrees Kelvin. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EOSID 
Type 
I 
Default 
none 
Card for the expansion of Specific Heat at Constant Pressure. Valid for T < 1000  0 K 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Cp1_0 
Cp1_1 
Cp1_2 
Cp1_3 
Cp1_4 
Type 
F 
Default 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
Card for the expansion of Specific Heat at Constant Pressure. Valid for T > 1000  0 K. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Cp2_0 
Cp2_1 
Cp2_2 
Cp2_3 
Cp2_4 
Type 
F 
Default 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0.
Card for the expansion of Specific Heat at Constant Volume. Valid for T < 1000  0 K 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Cv1_0 
Cv1_1 
Cv1_2 
Cv1_3 
Cv1_4 
Type 
F 
Default 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
Card for the expansion of Specific Heat at Constant Volume. Valid for T > 1000  0 K. 
  Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Cv2_0 
Cv2_1 
Cv2_2 
Cv2_3 
Cv2_4 
Type 
F 
Default 
0. 
F 
0. 
F 
0. 
F 
0. 
F 
0. 
  VARIABLE   
DESCRIPTION 
EOSID 
Equation of state identifier for the CESE solver. 
Cp1_0, …, 
Cp1_4 
Coefficients  of  temperature-dependent  specific  heat  at  constant 
pressure valid for T < 1000  0 K. 
Cp1(T) = Cp1_0 + Cp1_1 T + Cp1_2 T2 + Cp1_3 T3 + Cp1_4 T4 
Cp2_0, …, 
Cp2_4 
Coefficients  of  temperature-dependent  specific  heat  at  constant 
pressure valid for T > 1000  0 K. 
Cp2(T) = Cp2_0 + Cp2_1 T + Cp2_2 T2 + Cp2_3 T3 + Cp2_4 T4 
Cv1_0, …, 
Cv1_4 
Coefficients  of  temperature-dependent  specific  heat  at  constant 
volume  valid for T < 1000  0 K. 
Cv1(T) = Cv1_0 + Cv1_1 T + Cv1_2 T2 + Cv1_3 T3 + Cv1_4 T4 
Cv2_0, …, 
Cv2_4 
Coefficients  of  temperature-dependent  specific  heat  at  constant 
volume valid for T > 1000  0 K. 
Cv2(T) = Cv2_0 + Cv2_1 T + Cv2_2 T2 + Cv2_3 T3 + Cv2_4 T4
*CESE_EOS_INFLATOR2 
2.These coefficient expansions for the specific heats over two temperature ranges are 
See 
generated 
*CHEMISTRY_CONTROL_INFLATOR 
and 
*CHEMISTRY_INFLATOR_PROPERTIES for details related to running that solver.
inflator 
solver. 
model 
0-D 
the 
by
*CESE 
Purpose:  Provide  a  list  of  mechanics  solver  parts  that  are  not  involve  in  the  CESE  FSI 
calculation.  This is intended to be used as an efficiency measure for parts that will not 
involve significant FSI interactions with the CESE compressible fluid solver.. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID1 
PID2 
PID3 
PID4 
PID5 
PID6 
PID7 
PID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
PIDn 
DESCRIPTION 
IDs of mechanics parts that will be excluded from the FSI interaction
calculation with the CESE solver.
*CESE_INITIAL 
Purpose: Specify constant initial conditions (ICs) for flow variables at the centroid of each 
fluid element.  
  Card 1 
Variable 
Type 
Default 
1 
U 
F 
0 
2 
V 
F 
3 
W 
F 
4 
RH 
F 
5 
P 
F 
6 
T 
F 
0.0 
0.0 
1.225 
0.0 
0.0 
7 
8 
  VARIABLE   
DESCRIPTION 
U, V, W 
x-, y-, z-velocity components respectively 
density ρ 
pressure Ρ 
temperature Τ 
RHO 
P 
T 
Remarks: 
1.  Usually, only two of ρ, Ρ & Τ are needed to be specified (besides the velocity).  If all 
three are given, only ρ and Ρ will be used.  
2.  These  initial  condition  will  be  applied  in  those  elements  that  have  not  been 
assigned a value by *CESE_INITIAL_OPTION cards for individual elements or 
sets of elements.
*CESE_INITIAL_{OPTION} 
*CESE_INITIAL_{OPTION} 
Available options include: 
SET 
ELEMENT 
*CESE 
Purpose: Specify initial conditions for the flow variables at the centroid of each element in a 
set of elements or at the centroid of a single element. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
Variable 
EID/ESID 
Type 
I 
2 
U 
F 
3 
V 
F 
4 
W 
F 
5 
RHO 
F 
6 
P 
F 
7 
T 
F 
8 
Default 
none 
0.0 
0.0 
0.0 
1.225 
0.0 
0.0 
Remarks 
1 
1 
1 
  VARIABLE   
DESCRIPTION 
EID/ESID 
Solid element ID (EID) or solid element set ID (ESID) 
U, V, W 
x-, y-, z-velocity components respectively 
RHO 
density 
P 
T 
pressure 
temperature 
Remarks: 
1.  Usually, only two of ρ, Ρ & Τ are needed to be specified (besides the velocity).  If all 
three are given, only ρ and Ρ will be used. 
2.  The  priority  of  this  card  is  higher  than  *CESE_INITIAL,  i.e.,  if  an  element  is 
assigned an initial value by this card, *CESE_INITIAL will no longer apply to that 
element.
*CESE_INITIAL_CHEMISTRY 
Purpose:  Initializes the chemistry and fluid state in every element of the CESE mesh that 
has not already been initialized by one of the other *CESE_INITIAL_CHEMISTRY cards.  
This is only used when chemistry is being solved with the CESE solver. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CHEMID 
COMPID 
Type 
I 
I 
Default 
none 
none 
  Card 2 
1 
Variable 
UIC 
2 
VIC 
3 
4 
5 
WIC 
RHOIC 
PIC 
6 
TIC 
7 
HIC 
8 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
CHEMID 
Identifier of  chemistry control card to use. 
COMPID 
Identifier of chemical composition to use. 
UIC 
VIC 
WIC 
X-component of the fluid velocity. 
Y-component of the fluid velocity. 
Z-component of the fluid velocity. 
RHOIC 
Initial fluid density. 
PIC 
TIC 
Initial fluid pressure. 
Initial fluid temperature.
VARIABLE   
HIC 
DESCRIPTION 
Initial fluid enthalpy.  However, when CHEMID refers to a ZND 1-
step  reaction  card,  this  is  the  progressive  variable  (degree  of
combustion).
*CESE_INITIAL_CHEMISTRY_ELEMENT 
Purpose:    Initializes  the  chemistry  and  fluid  state  in  every  element  of  the  list  of  CESE 
elements.  This is only used when chemistry is being solved with the CESE solver. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CHEMID 
COMPID 
Type 
I 
I 
Default 
none 
none 
  Card 2 
1 
Variable 
UIC 
2 
VIC 
3 
4 
5 
WIC 
RHOIC 
PIC 
6 
TIC 
7 
HIC 
8 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
Element  List  Card.  Provide  as  many  cards  as  necessary.    This  input  ends  at  the  next 
keyword (“*”) card. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ELE1 
ELE2 
ELE3 
ELE4 
ELE5 
ELE6 
ELE7 
ELE8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
CHEMID 
Identifier of  chemistry control card to use. 
COMPID 
Identifier of chemical composition to use.
VARIABLE   
DESCRIPTION 
UIC 
VIC 
WIC 
X-component of the fluid velocity. 
Y-component of the fluid velocity. 
Z-component of the fluid velocity. 
RHOIC 
Initial fluid density. 
PIC 
TIC 
HIC 
Initial fluid pressure. 
Initial fluid temperature. 
Initial fluid enthalpy.  However, when CHEMID refers to a ZND 1-
step  reaction  card,  this  is  the  progressive  variable  (degree  of
combustion). 
ELE1, … 
User element numbers to initialize.
*CESE_INITIAL_CHEMISTRY_PART 
Purpose:  Initializes the chemistry and fluid state in every element of the specified CESE 
part that has not already been initialized by *CESE_INITIAL_CHEMISTRY_ELEMENT or 
*CESE_INITIAL_CHEMISTRY_SET  cards.    This  is  only  used  when  chemistry  is  being 
solved with the CESE solver. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PARTID 
CHEMID 
COMPID 
Type 
I 
I 
I 
Default 
none 
none 
none 
  Card 2 
1 
Variable 
UIC 
2 
VIC 
3 
4 
5 
WIC 
RHOIC 
PIC 
6 
TIC 
7 
HIC 
8 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
PARTID 
Identifier of the CESE part on which to initialize. 
CHEMID 
Identifier of chemistry control card to use. 
COMPID 
Identifier of chemical composition to use. 
UIC 
VIC 
WIC 
X-component of the fluid velocity. 
Y-component of the fluid velocity. 
Z-component of the fluid velocity. 
RHOIC 
Initial fluid density. 
PIC 
TIC 
2-62 (CESE) 
Initial fluid pressure.
VARIABLE   
HIC 
DESCRIPTION 
Initial fluid enthalpy.  However, when CHEMID refers to a ZND 1-
step  reaction  card,  this  is  the  progressive  variable  (degree  of
combustion).
*CESE_INITIAL_CHEMISTRY_SET 
Purpose:  Initializes the chemistry and fluid state in every element of the specified element 
set in the CESE mesh that has not already been initialized by *CESE_INITIAL_CHEM-
ISTRY_ELEMENT cards.  This is only used when chemistry is being solved with the CESE 
solver. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SETID 
CHEMID 
COMPID 
Type 
I 
I 
I 
Default 
none 
none 
none 
  Card 2 
1 
Variable 
UIC 
2 
VIC 
3 
4 
5 
WIC 
RHOIC 
PIC 
6 
TIC 
7 
HIC 
8 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
SETID 
Identifier of the CESE element set to initialize. 
CHEMID 
Identifier of  chemistry control card to use. 
COMPID 
Identifier of chemical composition to use. 
UIC 
VIC 
WIC 
X-component of the fluid velocity. 
Y-component of the fluid velocity. 
Z-component of the fluid velocity. 
RHOIC 
Initial fluid density. 
PIC 
TIC 
2-64 (CESE) 
Initial fluid pressure.
VARIABLE   
HIC 
DESCRIPTION 
Initial fluid enthalpy.  However, when CHEMID refers to a ZND 1-
step  reaction  card,  this  is  the  progressive  variable  (degree  of
combustion).
*CESE_INITIAL_CHEMISTRY_SET 
Purpose: Define the fluid (gas) properties in a viscous flow for the CESE solver.  
Material Definition Cards.  Include one card for each instance of this material type.  This 
input ends at the next keyword (“*”) card. 
4 
5 
6 
7 
8 
  Card 1 
1 
Variable 
MID 
2 
MU 
Type 
I 
F 
3 
K 
F 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
MID 
MU 
Material identifier 
Fluid dynamic viscosity.  For Air at 15 °C, MU =  1.81 × 10−5  
kg
ms⁄
K 
Thermal conductivity of the fluid 
Remarks: 
1.  The viscosity is only used viscous flows, so for inviscid flows, it is not necessary to 
define it.  The thermal conductivity is only used to calculate the heat transfer be-
tween the structure and the thermal solver when coupling is activated. 
2.  As with other solvers in LS-DYNA, the user is responsible for unit consistency.  
For example, if dimensionless variables are used, MU should be replaced by the 
corresponding dimensionless one.
*CESE 
Purpose: Define the fluid (gas) properties in a viscous flow for the CESE solver.  
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
Variable 
MID 
Type 
I 
2 
C1 
F 
3 
C2 
F 
4 
5 
6 
7 
8 
PRND 
F 
Default 
none 
1.458E-
6 
110.4 
0.72 
  VARIABLE   
DESCRIPTION 
MID 
Material identifier 
C1, C2 
Two coefficients in the Sutherland’s formula for viscosity, i.e., 
𝜇 =
𝐶1𝑇
𝑇 + 𝐶2
where C1 and C2 are constants for a given gas.  For example, for air
at moderate temperatures, 
𝐶1 = 1.458 × 10−6 kg msK
⁄
2⁄
,
𝐶2 = 110.4 K 
PRND 
The Prandtl Number (used to determine the coefficient of thermal
conductivity).  It is approximately constant for most gases.  For air at
standard conditions PRND = 0.72. 
Remarks: 
1.  C1 and C2 are only used to calculate the viscosity in viscous flows, so for inviscid 
flows, this material card is not needed.  The Prandtl number is used to extract the 
thermal conductivity, which is used when thermal coupling with the structure is 
activated. 
2.  As with other solvers in LS-DYNA, the user is responsible for unit consistency.  
For example, if dimensionless variables are used, C1 and C2 should be replaced by 
the corresponding dimensionless ones.
*CESE_MAT_002 
Purpose:  Define the fluid (gas) properties in a viscous flow for the CESE solver.  
Material Definition Cards.  Include one card for each instance of this material type.  This 
input ends at the next keyword (“*”) card. 
6 
7 
8 
  Card 1 
1 
2 
3 
Variable 
MID 
MU0 
SMU 
Type 
I 
F 
F 
4 
K0 
F 
5 
SK 
F 
Default 
none 
1.716E-5 
111. 
0.0241 
194.0 
  VARIABLE   
DESCRIPTION 
MID 
Material identifier 
MU0 / SMU 
Two coefficients appearing in the equation derived by combining
Sutherland’s formula with the Power law for dilute gases: 
𝜇0
= (
𝑇0
)
3 2⁄ 𝑇0 + 𝑆𝜇
𝑇 + 𝑆𝜇
. 
In  the  above,  MU0  and  SMU  are  parameters  characterizing  a
particular gas.  For example, for air at moderate temperatures, 
𝜇0 = 1.716 × 10−5 Ns m2⁄
,
𝑆𝜇 = 111 K 
K0/SK 
Two coefficients appearing in the equation derived by combining
Sutherland’s formula with the Power law for dilute gases: 
𝑘0
= (
𝑇0
)
3 2⁄ 𝑇0 + 𝑆𝑘
𝑇 + 𝑆𝑘
In the above, K0 and SK are parameters characterizing a particular
gas.  For example, for air at moderate temperatures, 
𝑘0 = 0.0241 W m⁄
,
𝑆𝑘 = 194 K 
Remarks: 
1.  The viscosity is only used viscous flows, so for inviscid flows, it is not necessary to 
define it.  The thermal conductivity is only used to calculate the heat transfer be-
tween the structure and the thermal solver when coupling is activated.
2.  As with other solvers in LS-DYNA, the user is responsible for unit consistency.  
For example, if dimensionless variables are used, MU should be replaced by the 
corresponding dimensionless one.
*CESE_PART 
Purpose: Define CESE solver parts, i.e., connect CESE material and EOS information.  
Part Cards.  Include one card for each CESE part.  This input ends at the next keyword 
(“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
MID 
EOSID 
Type 
I 
I 
I 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
PID 
MID 
Part identifier (must be different from any PID on a *PART card) 
Material identifier defined by a *CESE_MAT_… card 
EOSID 
Equation of state identifier defined by a *CESE_EOS_… card 
Remarks: 
1.  Since material coefficients are only used in viscous flows, the MID can be left blank 
for inviscid flows.
*CESE_SURFACE_MECHSSID_D3PLOT 
Purpose:  Identify the surfaces to be used in generating surface D3PLOT output for the 
CESE solver.  These surfaces must be on the outside of volume element parts that are in 
contact with the CESE fluid mesh.   The variables in question are  part of the CESE FSI 
solution process or of the CESE conjugate heat transfer solver. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
SurfaceLabel 
Type 
I 
Default 
none 
  VARIABLE   
SSID 
A 
none 
DESCRIPTION 
Mechanics  solver segment set ID that is in  contact with the fluid
CESE mesh. 
SurfaceLabel 
Name to use in d3plot output to identify the SSID for the LSPP user.
*CESE_SURFACE_MECHVARS_D3PLOT 
Purpose:  List of variables to output on the surfaces designated by the segment set IDs 
given in the *CESE_SURFACE_MECHSSID_D3PLOT cards.  Most of the allowed variables 
are defined only on the fluid-structure interface, and so the segment set IDs defining a 
portion of the fluid-structure interface must involve only segments (element faces) that are 
on the outside of volume element parts that are in contact with the CESE fluid mesh. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
  VARIABLE   
Output 
Quantity 
Output Quantity 
A 
none 
DESCRIPTION 
Descriptive phrase for  the mechanics surface variable to output for
the LSPP user.  Output will be done on all SSIDs selected by the
*CESE_SURFACE_MECHSSID_D3PLOT cards in the problem. 
Supported variables include: 
FLUID FSI FORCE 
FLUID FSI PRESSURE 
INTERFACE TEMPERATURE 
SOLID INTERFACE HEAT FLUX 
FLUID INTERFACE HEAT FLUX 
INTERFACE HEAT FLUX RATE 
SOLID INTERFACE DISPLACEMENT 
SOLID INTERFACE VELOCITY 
SOLID INTERFACE ACCELERATION 
Force, displacement, velocity, and acceleration are output as vector
quantities.  The rest of the variables are scalar quantities.  The fluxes
are in the normal direction to the fluid/structure interface, with the
heat fluxes relative to the normal pointing into the structure.
*CHEMISTRY 
The keyword *CHEMISTRY is used to access chemistry databases that include Chemkin-
based descriptions of a chemical model, as well as to select a method of solving the model.  
The keyword cards in this section are defined in alphabetical order: 
*CHEMISTRY_COMPOSITION 
*CHEMISTRY_CONTROL_0D 
*CHEMISTRY_CONTROL_1D
†
*CHEMISTRY_CONTROL_CSP 
*CHEMISTRY_CONTROL_FULL 
*CHEMISTRY_CONTROL_INFLATOR
†
*CHEMISTRY_CONTROL_TBX 
*CHEMISTRY_CONTROL_ZND
†
*CHEMISTRY_DET_INITIATION
†
*CHEMISTRY_INFLATOR_PROPERTIES
†
*CHEMISTRY_MODEL 
*CHEMISTRY_PATH 
†: Card may be used only once in a given model 
An additional option “_TITLE” may be appended to all *CHEMISTRY keywords.  If this 
option  is  used,  then  an  80  character  string  is  read  as  a  title  from  the  first  card  of  that 
keyword's input.  At present, LS-DYNA does not make use of the title.  Inclusion of titles 
gives greater clarity to input decks. 
In order to use one of the chemistry solvers, the input must include at least one *CHEM-
ISTRY_MODEL card.  For each spatial region containing a different chemical composition, 
at least one *CHEMISTRY_COMPOSITION card is required. 
The *CHEMISTRY_CONTROL_0D card is intended to be used in a standalone fashion to 
verify the validity of a given chemistry model.  This model includes the total number of 
species and all elementary reactions with their Arrhenius rate parameters.  For instance, 
this solver could be used to check the induction time of the model.
The  *CHEMISTRY_CONTROL_1D,  *CHEMISTRY_DET_INITIATION,  and  *CHEM-
ISTRY_CONTROL_ZND cards are intended to provide a one-dimensional initialization to 
a 2D or 3D chemically-reacting flow. 
In order to perform a full, general purpose chemistry calculation in 2D or 3D, the *CHEM-
ISTRY_CONTROL_FULL card should be used. 
The *CHEMISTRY_CONTROL_CSP card is an option for reducing the number of species 
and reactions that are used in a general purpose chemistry calculation.  Other reduction 
mechanisms are planned for the future. 
An airbag inflator model is available with *CHEMISTRY_CONTROL_INFLATOR along 
with *CHEMISTRY_INFLATOR_PROPERTIES and a chemistry model that is referenced 
via  three  chemical  compositions.    This  involves  zero-dimensional  modeling,  with 
pyrotechnic inflator, and cold and hot flow hybrid inflator options. 
The *CHEMISTRY_CONTROL_TBX card is intended for use only in a stochastic particle 
model, where the *STOCHASTIC_TBX_PARTICLES card is used.
*CHEMISTRY 
Purpose:  Provides a general way to specify a chemical composition via a list of species 
mole numbers in the context of a Chemkin database model. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
MODELID 
Type 
I 
I 
Default 
none 
none 
Species  List  Card.  Provide  as  many  cards  as  necessary.    This  input  ends  at  the  next 
keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MOLFR 
Type 
F 
Default 
none 
SPECIES 
A 
none 
  VARIABLE   
DESCRIPTION 
ID 
A unique identifier among all chemistry compositions. 
MODELID 
Identifier of a Chemkin-compatible chemistry model. 
MOLFR 
SPECIES 
The number of moles  corresponding to the species named in the
SPECIES field.  But if used with a *STOCHASTIC_TBX_PARTICLES
card,  it  is  the  molar  concentration  of  the  species  (in  units  of
moles/[length]3, where “[length]” is the user’s length unit). 
The Chemkin-compatible name of a chemical species that is defined
in  the  chemistry  model  identified  by  MODELID  .
*CHEMISTRY_CONTROL_0D 
Purpose:    Performs  a  zero-dimensional  isotropic  chemistry  calculation  that  operates 
standalone (does not call the CESE solver).  This is for ISOBARIC or ISOCHORIC cases. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
COMPID 
SOLTYP 
PLOTDT  CSP_SEL
Type 
I 
I 
I 
F 
Default 
none 
none 
none 
1.0e-6 
Remarks 
  Card 2 
Variable 
1 
DT 
2 
3 
TLIMIT 
TIC 
4 
PIC 
I 
0 
1 
5 
RIC 
7 
8 
6 
EIC 
Type 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
CSP Parameters Card. Include cards for each chemical species in the following format 
when CSP_SEL.GT.0.  This input ends at the next keyword (“*”) card. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
AMPL 
YCUT 
Type 
F 
F 
Default 
none 
none 
  VARIABLE   
DESCRIPTION 
ID 
Identifier for this 0D computation.
VARIABLE   
DESCRIPTION 
COMPID 
Chemical composition identifier of composition to use. 
SOLTYP 
Type of 0D calculation: 
EQ.1: Isochoric 
EQ.2: Isobaric 
PLOTDT 
Simulation time interval for output both to the screen and to the
isocom.csv file.  This file can be loaded into LS-PREPOST for curve 
plotting using the x-y plot facility. 
CSP_SEL 
CSP solver option: 
EQ.0: Do  not  use  the  CSP  solver,  and  ignore  the  AMPL  and 
YCUT parameters (default). 
GT.0:  Use the CSP solver, with the AMPL and YCUT parameters.
DT 
Initial time step 
TLIMIT 
Time limit for the simulation 
Initial temperature 
Initial pressure 
Initial density 
Initial internal energy 
Relative accuracy for the mass fraction of a chemical species in the
Chemkin input file. 
Absolute accuracy for the mass fraction of a chemical species in the
Chemkin input file. 
TIC 
PIC 
RIC 
EIC 
AMPL 
YCUT 
Remarks: 
1. 
If CSP_SEL.GT.0, then instead of using the full chemistry solver, the computational 
singular perturbation (CSP) method solver is used.
*CHEMISTRY_CONTROL_1D 
Purpose:  Loads a previously-computed one-dimensional detonation.  It is then available 
for use in the CESE solver for initializing a computation.  In the product regions, this card 
overrides the initialization of the *CESE_INITIAL_CHEMISTRY_… cards. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
XYZD 
DETDIR  CSP_SEL
Type 
I 
F 
I 
Default 
none 
none 
none 
Remarks 
I 
0 
1 
One-Dimensional Solution LSDA Input File Card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
FILE 
A 
CSP Parameters Card Include cards for each chemical species in the following format 
when CSP_SEL  >  0.  This input ends at the next keyword (“*”) card. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
AMPL 
YCUT 
Type 
F 
F 
Default 
none 
none 
  VARIABLE   
DESCRIPTION 
ID 
Identifier for this one-dimensional detonation solution. 
XYZD 
Position of the detonation front in the DETDIR direction.
VARIABLE   
DESCRIPTION 
DETDIR 
Detonation propagation direction 
EQ.1:  𝑥 
EQ.2:  𝑦 
EQ.3:  𝑧 
CSP_SEL 
CSP solver option: 
EQ.0:  Do  not  use  the  CSP  solver,  and  ignore  the  AMPL  and 
YCUT parameters (default). 
GT.0:  Use the CSP solver, with the AMPL and YCUT parameters.
FILE 
Name of the LSDA file containing the one-dimensional solution. 
Relative accuracy for the mass fraction of a chemical species in the
chemkin input file. 
Absolute accuracy for the mass fraction of a chemical species in the
chemkin input file. 
AMPL 
YCUT 
Remarks: 
1. 
If CSP_SEL > 0, then instead of using the full chemistry solver, the computational 
singular perturbation (CSP) method solver is used.
*CHEMISTRY_CONTROL_CSP 
Purpose:  Computes reduced chemistry for a specified Chemkin chemistry model using the 
Computational Singular Perturbation (CSP) method.  This card can be used for general-
purpose chemical reaction calculations. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
IERROPT 
Type 
I 
I 
Default 
none 
none 
CSP Parameters Card. Include cards for each chemical species in the following format as 
indicated by the value of IERROPT.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
AMPL 
YCUT 
Type 
F 
F 
Default 
none 
none 
  VARIABLE   
DESCRIPTION 
ID 
Identifier for this computational singular perturbation solver. 
IERROPT 
Selector: 
EQ.0:  AMPL  and  YCUT  values  for  all  chemical  species  are
required. 
EQ.1:  One CSP Parameter Card should be provided, and it will
be used for all species. 
AMPL 
YCUT 
Relative accuracy for the mass fraction of a chemical species in the
Chemkin input file. 
Absolute accuracy for the mass fraction of a chemical species in the
Chemkin input file.
*CHEMISTRY_CONTROL_FULL 
Purpose:  Computes the full chemistry specified by a Chemkin chemistry model.  This card 
can be used for general-purpose chemical reaction calculations. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
ERRLIM 
RHOMIN 
TMIN 
Type 
I 
F 
F 
F 
Default 
none 
none 
0.0 
0.0 
  VARIABLE   
DESCRIPTION 
ID 
Identifier for this full chemistry calculation. 
ERRLIM 
Error tolerance for the full chemistry calculation. 
RHOMIN 
TMIN 
Minimum  fluid  density  above  which  chemical  reactions  are
computed. 
Minimum  temperature  above  which  chemical  reactions  are 
computed.
*CHEMISTRY_CONTROL_INFLATOR 
Purpose:  Provide the required properties of an inflator model for airbag inflation. 
Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MODEL  OUT_TYPE  TRUNTIM
DELT 
PTIME 
Type 
Remarks 
I 
1 
I 
F 
F 
F 
2,4 
Inflator Output Database File (an ASCII file) Card. 
Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
FILE 
A 
Densities for Condensed Species. Include as many cards as needed.  This input ends at 
the next keyword (“*”) card. 
Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DENSITY 
Species Name 
Type 
F 
Default 
none 
Remark 
  VARIABLE   
3-10 (CHEMISTRY) 
A 
none
VARIABLE   
DESCRIPTION 
MODEL 
Type of inflator model to compute. 
EQ.1: 
EQ.2: 
Pyrotechnic model 
Hybrid  model  with  cold  flow  option  in  the  gas
chamber 
EQ.3: 
Hybrid model with heat flow in the gas chamber 
OUT_TYPE 
Selects  the  output  file  format  that  will  be  used  in  an  airbag
simulation. 
EQ.0: 
EQ.1: 
EQ.2: 
EQ.3:  
EQ.4:  
Screen output  
CESE compressible flow solver (default) 
ALE solver 
CPM solver (with 2nd-order expansion of C p ) 
CPM solver (with 4th-order expansion of C p ) 
TRUNTIM 
Total run time. 
DELT 
Delta(t) to use in the model calculation. 
PTIME 
Time interval for output of time history data to FILE. 
FILE 
Name of the ASCII file in which to write the time history data and
other data output by the inflator simulation. 
DENSITY 
Density of a condensed-phase species present in the inflator. 
Chemkin-compatible name of a condensed-phase species. 
Species 
Name 
Remarks: 
1. 
If MODEL = 3, the solution of an elementary reaction system is required for the 
finite-rate chemistry in the gas chamber. 
2.  Output  file  includes  all  of  the  necessary  thermodynamics  variables  and  load 
curves for the species mass flow rate, temperature, and density curve.  This will 
make it possible to generate the velocity curve which is required by each solver 
that carries out an airbag simulation.
3.  At least one of these cards will be input if condensed-phase species are present 
during the propellant combustion.  In this case, the user must specify each con-
densed-phase density.  This density is then used to compute the volume fractions 
in both the combustion and gas chamber, where the energy equations are needed. 
4. 
If  OUT_TYPE = 0,  the  propellant  information  will  be  displayed  on  the  screen, 
including total mass, remaining mass percentage, and mass burning rate versus 
time.  With this option, the user can quickly see the effect of changing the parame-
ters on the first three *CHEMISTRY_INFLATOR_PROPERTIES cards.
*CHEMISTRY 
Purpose:  Specify a chemistry solver for use in conjunction with stochastic TBX particles.  
This is intended only for modeling the second phase of an explosion where the explosive 
has embedded metal (aluminum) particles that are too large to have burned in the first 
phase of the explosion. 
This  chemistry  card  points  to  a  *CHEMISTRY_MODEL  card  (via  IDCHEM)  with  its 
associated *CHEMISTRY_COMPOSITION cards to set up the initial conditions.  That is, it 
establishes the spatial distribution of the species in the model. 
It is assumed that there is no chemical reaction rate information in the chemistry model 
files.  This is done since a special chemical reaction mechanism is implemented for TBX 
modeling.  If particles other than solid aluminum particles are embedded in the explosive, 
then another burn model has to be implemented. 
Surface Part Card.  Card 1 format used when the PART keyword option is active. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
IDCHEM 
USEPAR 
Type 
I 
Default 
none 
I 
1 
  VARIABLE   
DESCRIPTION 
IDCHEM 
Identifier for this chemistry solver. 
USEPAR 
Coupling flag indicating if a *STOCHASTIC_TBX_PARTICLES card 
is provided for this model: 
EQ.1: uses a *STOCHASTIC_TBX_PARTICLES card (default). 
EQ.0: does not use such a card.
*CHEMISTRY_CONTROL_ZND 
Purpose:  Computes the one-dimensional reduced chemistry of a ZND model.  It is then 
used in the initialization of the chemistry part of the CESE solver.  When this card is used, 
the *CESE_INITIAL_CHEMISTRY… cards must specify the progressive variable (degree of 
combustion) in the HIC field. 
  Card 1 
Variable 
1 
ID 
Type 
I 
Default 
none 
  Card 2 
Variable 
Type 
1 
F 
F 
2 
3 
4 
5 
6 
7 
8 
2 
EPLUS 
3 
Q0 
4 
5 
6 
7 
8 
GAM 
XYZD 
DETDIR 
F 
F 
F 
F 
I 
Default 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
ID 
F 
Identifier for this full chemistry calculation. 
Overdriven factor 
EPLUS 
EPLUS parameter of the ZND model. 
Q0 
Q0 parameter of the ZND model. 
GAM 
XYZD 
GAM parameter of the ZND model. 
Position of the detonation front in the DETDIR direction. 
DETDIR 
Detonation propagation direction (1 => X; 2 => Y; 3 => Z)
*CHEMISTRY_DET_INITIATION 
Purpose:    Performs  a  one-dimensional  detonation  calculation  based  upon  a  chemical 
composition and initial conditions.  It is then available for use immediately in the CESE 
solver for initializing a computation, or it can be subsequently used by the *CHEMISTRY_-
CONTROL_1D  card  in  a  later  run.    In  the  product  regions,  this  card  overrides  the 
initialization of the *CESE_INITIAL_CHEMISTRY… cards. 
  Card 1 
Variable 
1 
ID 
2 
3 
4 
5 
6 
7 
8 
COMPID 
NMESH 
DLEN 
CFL 
TLIMIT 
XYZD 
DETDIR 
Type 
I 
I 
I 
F 
F 
F 
F 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
LSDA Output File Card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
FILE 
A 
  VARIABLE   
DESCRIPTION 
ID 
Identifier for this one-dimensional detonation computation. 
COMPID 
Chemical composition identifier of composition to use. 
NMESH 
Number of equal-width elements in the one-dimensional domain.
DLEN 
Length of the one-dimensional domain. 
CFL 
Time-step limiting factor. 
TLIMIT 
Time limit for the simulation 
XYZD 
Position of the detonation front in the DETDIR direction. 
DETDIR 
Detonation propagation direction (1 => X; 2 => Y; 3 => Z)
VARIABLE   
FILE 
DESCRIPTION 
Name  of  the  LSDA  file  in  which  to  write  the  one-dimensional 
solution.
*CHEMISTRY_INFLATOR_PROPERTIES 
Purpose:  Provide the required properties of an inflator model. 
Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
COMP_ID 
PDIA 
PHEIGHT 
PMASS  TOTMASS
Type 
Remarks 
I 
1 
F 
F 
F 
F 
Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TFLAME 
PINDEX 
A0 
TDELAY  RISETIME
Type 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
None 
Combustion Chamber Parameter Card. 
Card 3 
1 
2 
3 
4 
Variable 
COMP1ID 
VOL1 
AREA1 
CD1 
Type 
I 
F 
F 
F 
5 
P1 
F 
6 
7 
8 
T1 
DELP1 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none
Gas Plenum Parameter Card. 
Card 4 
1 
2 
3 
4 
Variable 
COMP2ID 
VOL2 
AREA2 
CD2 
Type 
I 
F 
F 
F 
5 
P2 
F 
6 
7 
8 
T2 
DELP2 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
Tank Parameter Card. 
Card 5 
1 
2 
3 
Variable 
COMP3ID 
VOL3 
P3 
Type 
I 
F 
F 
4 
T3 
F 
Default 
none 
none 
none 
none 
5 
6 
7 
8 
  VARIABLE   
COMP_ID 
DESCRIPTION 
Chemical composition identifier of the composition for the steady-
state propellant combustion . 
PDIA 
Propellant diameter. 
PHEIGHT 
Propellant height. 
PMASS 
Individual cylinder propellant mass. 
TOTMASS 
Total propellant mass. 
TFLAME 
Adiabatic flame temperature. 
PINDEX  
Power of the pressure in rate of burn model. 
A0 
Steady-state constant. 
TDELAY  
Ignition time delay.
VARIABLE   
DESCRIPTION 
RISETIME 
Rise time. 
COMP1ID 
Chemical  composition  identifier  of  composition  to  use  in  the
combustion chamber. 
VOL1 
Volume of the combustion chamber. 
AREA1 
Area of the combustion chamber. 
CD1 
Discharge coefficient of the combustion chamber. 
P1 
T1 
Pressure in the combustion chamber. 
Temperature in the combustion chamber. 
DELP1 
Rupture pressure in the combustion chamber. 
COMP2ID 
Chemical composition identifier of composition to use in the gas
plenum. 
VOL2 
Volume of the gas plenum. 
AREA2 
Area of the gas plenum. 
CD2 
Discharge coefficient of the gas plenum. 
P2 
T2 
Pressure in the gas plenum. 
Temperature in the gas plenum. 
DELP2 
Rupture pressure in the gas plenum. 
COMP3ID 
Chemical composition identifier of composition to use in the tank.
VOL3 
Volume of the tank. 
P3 
T3 
Pressure in the tank. 
Temperature in the tank. 
Remarks: 
1.  The propellant composition can be obtained by running a chemical equilibrium 
program such as NASA CEA, the CHEETAH code, or the PEP code.  LSTC pro-
vides a modified version of the PEP code along with documentation for users; it is 
available upon request.
*CHEMISTRY 
Purpose:  Identifies the files that define a Chemkin chemistry model. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  MODELID 
JACSEL 
ERRLIM 
Type 
I 
Default 
none 
I 
1 
F 
1.0e-3 
Chemkin Input File Card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
FILE1 
A 
Thermodynamics Database File Card. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
FILE2 
A 
Transport Properties Database File Card. 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
FILE3 
A 
  VARIABLE   
DESCRIPTION 
MODELID 
Identifier for this Chemkin-based chemistry model..
VARIABLE   
DESCRIPTION 
JACSEL 
Selects the form of the Jacobian matrix for use in the source term.
EQ.1: Fully implicit (default) 
EQ.2: Simplified implicit 
ERRLIM 
Allowed error in element balance in a chemical reaction. 
FILE1 
FILE2 
FILE3 
Name of the file containing the Chemkin-compatible input. 
Name  of  the  file  containing  the  chemistry  thermodynamics 
database. 
Name  of  the  file  containing  the  chemistry  transport  properties 
database.
*CHEMISTRY 
Purpose:  To specify one or more search paths to look for chemistry database files. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
DIR 
A 
  VARIABLE   
DESCRIPTION 
DIR 
Directory path to add to the search set.
*EM 
The *EM keyword cards provide input for a new electromagnetism module for solving 3D 
eddy-current, inductive heating or resistive heating problems, coupled with mechanical 
and thermal solvers.  Typical applications include magnetic metal forming and welding.  A 
boundary element method in the air is coupled to finite elements in the conductor in order 
to avoid meshing the air. 
*EM_2DAXI 
*EM_BOUNDARY 
*EM_CIRCUIT 
*EM_CIRCUIT_CONNECT 
*EM_CIRCUIT_RANDLE 
*EM_CIRCUIT_ROGO 
*EM_CONTACT 
*EM_CONTACT_RESISTANCE 
*EM_CONTROL 
*EM_CONTROL_CONTACT 
*EM_CONTROL_SWITCH 
*EM_CONTROL_SWITCH_CONTACT 
*EM_CONTROL_TIMESTEP 
*EM_DATABASE_CIRCUIT 
*EM_DATABASE_CIRCUIT0D 
*EM_DATABASE_ELOUT 
*EM_DATABASE_FIELDLINE 
*EM_DATABASE_GLOBALENERGY 
*EM_DATABASE_NODOUT 
*EM_DATABASE_PARTDATA
*EM_DATABASE_POINTOUT 
*EM_DATABASE_ROGO 
*EM_DATABASE_TIMESTEP 
*EM_EOS_BURGESS 
*EM_EOS_MEADON 
*EM_EOS_PERMEABILITY 
*EM_EOS_TABULATED1 
*EM_EOS_TABULATED2 
*EM_EXTERNAL_FIELD 
*EM_ISOPOTENTIAL 
*EM_ISOPOTENTIAL_CONNECT 
*EM_MAT_001 
*EM_MAT_002 
*EM_MAT_003 
*EM_MAT_004 
*EM_OUTPUT 
*EM_POINT_SET 
*EM_RANDLE_SHORT 
*EM_ROTATION_AXIS 
*EM_SOLVER_BEM 
*EM_SOLVER_BEMMAT 
*EM_SOLVER_FEM 
*EM_SOLVER_FEMBEM 
*EM_VOLTAGE_DROP
*EM 
Purpose:  Sets up the electromagnetism solver as 2D axisymmetric instead of 3D, on a given 
part, in order to save computational time as well as memory. 
The electromagnetism is solved in 2D on a given cross section of the part (defined by a 
segment set), with a symmetry axis defined by its direction (at this time, it can be the 𝑥, 𝑦, 
or 𝑧 axis).  The EM forces and Joule heating are then computed over the full 3D part by 
rotations.  The part needs to be compatible with the symmetry, i.e.  each node in the part 
needs to be the child of a parent node on the segment set, by a rotation around the axis.  
Only the conductor parts (with a *EM_MAT_… of type 2 or 4) should be defined as 2D 
axisymmetric. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
SSID 
STARSSID ENDSSID  NUMSEC 
Type 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
Part ID of the part to be solved using 2D axisymmetry 
Segment Set ID : Segment that will define the 2D cross section of the
part where the EM field is solved 
Used  by  the  2D  axisymmetric  solver  to  make  the  connection
between two corresponding boundaries on each side of a slice when
the model is a slice of the full 360 circle. 
Number of Sectors.  This field gives the ratio of the full circle to the 
angular extension of the mesh.  This has to be a power of two.  For
example, NUMSEC = 4 means that the mesh of the part represents 
one fourth of the total circle.  If this value is set to 0, then the value
from *EM_ROTATION_AXIS is used instead. 
PID 
SSID 
STARSSID, 
ENDSSID 
NUMSEC 
Remarks: 
1.  At this time, either all or none of the conductor parts should be 2D axisymmetric.  
In the future, a mix between 2D axisymmetric and 3D parts will be allowed.
*EM_BOUNDARY 
Purpose:  Define some boundary conditions for the electromagnetism problems. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SSID 
BTYPE 
Type 
I 
I 
Default 
none 
none 
  VARIABLE   
DESCRIPTION 
SSID 
Segment Set Id 
BTYPE 
EQ.9: The faces of this segment set are eliminated from the BEM 
calculations (used for example for the rear or side faces of a
workpiece).
Available options include 
SOURCE 
Purpose:  Define an electrical circuit. 
*EM 
For the SOURCE option, the current will be considered uniform in the circuit.  This can be 
useful in order to save computational time in cases with a low frequency current and where 
the diffusion of the EM fields is a very fast process.  This option is in contrast with the 
general case where the current density in a circuit is completed in accordance with the 
solver type defined in EMSOL of *EM_CONTROL.  For example, if an eddy current solver 
is selected, the diffusion of the current in the circuit is taken into account. 
  Card 1 
1 
2 
3 
Variable 
CIRCID 
CIRCTYP 
LCID 
4 
R/F 
5 
L/A 
6 
C/to 
Type 
I 
I 
I 
F 
F 
F 
7 
V0 
F 
8 
T0 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
0. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SIDCURR 
SIDVIN 
SIDVOUT 
PARTID 
Type 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
CIRCID 
Circuit ID
VARIABLE   
DESCRIPTION 
CIRCTYP 
Circuit type: 
EQ.1:  Imposed current vs time defined by a load curve. 
EQ.2:  Imposed voltage vs time defined by a load curve. 
EQ.3:  R, L, C, V0 circuit. 
EQ.11:  Imposed current defined by an amplitude A, frequency F
and initial time 𝑡0: 𝐼 = 𝐴sin[2𝜋𝐹(𝑡 − 𝑡0)]
EQ.12:  Imposed voltage defined by an amplitude A, frequency F
and initial time 𝑡0: 𝑉 = 𝐴sin[2𝜋𝐹(𝑡 − 𝑡0)] 
EQ.21:  Imposed current defined by a load curve over one period 
and a frequency F 
EQ.22:  Imposed voltage defined by a load curve over one period
and a frequency F 
Load curve ID for CIRCTYP = 1, 2, 21 or 22 
Value of the circuit resistance for CIRCTYP = 3 
Value of the Frequency for CIRCTYP = 11, 12, 21 or 22 
Value of the circuit inductance for CIRCTYP = 3 
Value  of  the  Amplitude  for  CIRCTYP =  11  or  12.    To  have  the 
amplitude defined by a load curve, a negative value can be entered
and the solver will look for the corresponding Load Curve ID. 
Value of the circuit capacity for CIRCTYP = 3 
Value of the initial time t0 for CIRCTYP = 11 or 12 
Value of the circuit initial voltage for CIRCTYP = 3. 
Starting time for CIRCTYPE = 3.  Default is at the beginning of the 
run. 
Segment set ID for the current.  It uses the orientation given by the
normal of the segments.  To use the opposite orientation, use a '–' 
(minus) sign in front of the segment set id. 
CIRCTYP.EQ.1/11/21: The  current  is  imposed  through  this 
CIRCTYP.EQ.3: 
segment set 
the  circuit 
The  current  needed  by 
equations is measured through this seg-
ment set. 
LCID 
R/F 
L/A 
C/t0 
V0 
T0 
SIDCURR
SIDVIN 
*EM 
DESCRIPTION 
Segment  set  ID  for  input  voltage  or  input  current  when
CIRCTYP.EQ.2/3/12/22 and CIRCTYP.EQ 1/11/21 respectively.  It
is  considered  to  be  oriented  as  going  into  the  structural  mesh, 
irrespective of the orientation of the segment. 
SIDVOUT 
Segment  set  ID  for  output  voltage  or  output  current  when
CIRCTYP = 2/3/12/22 and CIRCTYP = 1/11/21 respectively.  It is 
considered  to  be  oriented  as  going  out  of  the  structural  mesh, 
irrespective of the orientation of the segment. 
PARTID 
Part ID associated to the Circuit.  It can be any part ID associated to
the circuit.
Circuit Type (CIRCTYP) 
Variable 
  1: Current 
 Imposed 
 Imposed
  2: Voltage 
3: R, L, C 
11: F, A, t0 
12: F, A, t0 
LCID 
R/L/C/V0 
F 
A/t0 
SIDCURR 
SIDVIN 
SIDVOUT 
PARTID 
M 
- 
- 
- 
M 
M* 
M* 
M 
M 
- 
- 
- 
O 
M 
M 
M 
Variable 
21: LCID, F 
22 : LCID, F 
LCID 
R/L/C/V0 
F 
A/t0 
SIDCURR 
SIDVIN 
SIDVOUT 
PARTID 
M 
- 
M 
- 
M 
M* 
M* 
M 
M 
- 
M 
- 
O 
M 
M 
M 
- 
M 
- 
- 
M 
M 
M 
M 
- 
- 
- 
- 
- 
- 
- 
- 
- 
- 
M 
M 
M 
M* 
M* 
M 
- 
- 
- 
- 
- 
- 
- 
- 
- 
- 
M 
M 
O 
M 
M 
M 
- 
- 
- 
- 
- 
- 
- 
- 
Table 4-1.  Correspondence between circuit type and card entries.  “M” 
indicates mandatory, “M*” mandatory with exceptions , 
“O” indicates optional, and “-” indicates ignored. 
Remarks: 
1.  When defining a circuit with an imposed current (type 1, 11 or 21) in cases of a 
closed loop geometry (torus), SIDVIN and SIDVOUT cannot be defined and thus, 
only SIDCURR is necessary. 
2.  When defining a circuit with an imposed tension (type 2, 12, 22), it is possible to 
also define SIDCURR.  This can be useful in circuits where various flow paths are
possible  for  the  current  in  order  to  force  the  entire  current  to  go  through 
SIDCURR. 
3.  Circuit types 21 and 22 are for cases where the periodic current/tension does not 
exactly follow a perfect sinusoidal.  The user has to provide the shape of the cur-
rent/tension over one period through a LCID as well as the frequency.
*EM_CIRCUIT 
Purpose:  This keyword connects several circuits together by imposing a linear constraint 
on the global currents of circuit pairs 
This is especially useful for 2D axisymmetric models involving spiral or helical coils. 
𝑐1𝑖1 + 𝑐2𝑖2 = 0. 
  Card 1 
1 
2 
3 
4 
Variable 
CONID 
CONTYPE 
CIRC1 
CIRC2 
Type 
I 
I 
I 
I 
5 
C1 
F 
6 
C2 
F 
7 
8 
Default 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
CONID 
Id of the Circuit Connect 
CONTYPE 
Type  of  connection  between  circuits.    For  the  moment,  it  is  only
possible to combine circuits by imposing a linear constraint on the
global current (=1). 
C1/C2 
Values of the linear constraints if CONTYPE = 1.
*EM 
Purpose: define the distributed Randle circuit parameters for a unit Randle cell. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RDLID 
RDLTYPE  RDLAREA
ISSID1 
ISSID2 
SEPPART  ANOPART  CATPART
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 2 
Variable 
Type 
1 
Q 
F 
2 
3 
4 
5 
6 
7 
8 
CQ 
SOCINIT  SOCTOU 
F 
F 
F 
Default 
none 
none 
none 
none 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
R0CHA 
R0DIS 
R10CHA 
R10DIS 
C10CHA 
C10DIS 
Type 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TEMP 
FRTHERM  R0TOTH 
DUDT 
TEMPU 
Type 
F 
I 
I 
F 
I 
Default 
none 
none 
none 
none 
none
Card 5 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  USESOCS  TAUSOCS  SICSLCID
Type 
I 
F 
I 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
RDLID 
Id of the Randle Cell 
RDLTYPE 
Type of Randle Cell 
RDLAREA 
Randle Area: 
EQ.0: Default.The parameters are not scaled by area factors. 
EQ.1:  The parameters are per unit area and will be scaled in each
Randle circuit by a factor depending on the local area of the 
circuit. 
EQ.2: The parameters are defined for the whole unit cell and will
be scaled in each Randle circuit by a factor depending on
the local area of the circuit and the global area of the cell.
ISSID1 
ISSID2 
Segment set ID defining the anode side on the current collector. 
Segment set ID defining the cathode side on the current collector.
SEPPART 
Separator Part ID 
ANOPART 
Anode Part ID 
CATPART 
Cathode Part ID 
Q 
CQ 
Unit cell capacity. 
SOC conversion factor (%/s), known to be equal to 1/36 in S.I units.
SOCINIT 
Initial state of charge of the unit cell.
VARIABLE   
SOCTOU 
DESCRIPTION 
Constant  value  if  positive  or  load  curve  ID  if  negative  integer
defining the equilibrium voltage (OCV) as a function of the state of
charge (SOC). 
R0CHA/ 
R10CHA/ 
C10CHA 
Constant  if  positive  value  or  load  curve  or  table  id  (if  negative
integer) defining r0/r10/c10 when the current flows in the charge
direction as a function of: 
-SOC if load curve 
-SOC and Temperature if table. 
R0DIS/ 
R10DIS/ 
C10DIS 
Constant  if  positive  value  or  load  curve  or  table  id  (if  negative
integer)  defining  r0/r10/c10  when  the  current  flows  in  the
discharge direction as a function of: 
-SOC if load curve 
-SOC and Temperature if table. 
TEMP 
Constant temperature value used for the Randle circuit parameters 
in case there is no coupling with the thermal solver (FRTHERM = 0)
FRTHERM 
From Thermal : 
EQ.0: The temperature used in the Randle circuit parameters is
TEMP 
EQ.1:  The temperature used in the Randle circuit parameter is the
temperature from the thermal solver. 
R0TOTH 
R0 to Thermal : 
EQ.0: The joule heating in the resistance r0 is not added to the
thermal solver 
EQ.1:  The  joule  heating  in  the  resistance  r0  is  added  to  the
thermal solver 
DUDT 
If negative integer, load curve ID of the reversible heat as a function 
of SOC. 
TEMPU 
Temperature Unit : 
EQ.0: The temperature is in Celsius 
EQ.1:  The Temperature is in Kelvin
VARIABLE   
DESCRIPTION 
USESOCS 
Use SOC shift  : 
EQ.0: Don't use the added SOCshift 
EQ.1:  Use the added SOCshift 
TAUSOCS 
Damping time in the SOCshift equation  
SOCSLCID 
Load curve giving f(i) where I is the total current in the unit cell 
Remarks: 
1.  Sometimes,  an  extra  term  called  SOCshift  (or  SocS)  can  be  added  at  high  rate 
discharges to account for diffusion limitations.  The SOCshift is added to SOC for 
the  calculation  of  the  OCV  u(SOC+SOCshift)  and  r0(Soc+SOCshift).    SOCshift 
satisfies the following equation: 
d(SOCshift)/dt + SOCshift/tau = f(i(t))/tau 
with SOCshift(t = 0)=0
*EM 
Purpose:  Define Rogowsky coils to measure a global current vs time through a segment set 
or a node set. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ROGID 
SETID 
SETTYPE  CURTYP 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION 
ROGID 
Rogowsky coil ID 
SETID 
Segment or node set ID 
SETTYPE 
Type of set: 
EQ.1: Segment set 
EQ.2: Node set (not available yet} 
CURTYP 
Type of current measured: 
EQ.1: Volume current 
EQ.2: Surface current (not available yet} 
EQ.3: Magnetic field flow (B field times Area) 
Remarks: 
1.  An ASCII file “em_rogo_xxx” , with xxx representing the rogoId, is generated for 
each *EM_CIRCUIT_ROGO card giving the value of the current or the magnetic 
field vs time.
*EM_CONTACT 
Purpose:    Optional  card  used  for  defining  and  specifying  options  on  electromagnetic 
contacts  between  two  sets  of  parts.    Generally  used  with  the  *EM_CONTACT_RESIS-
TANCE card.  Fields left empty on this card default to the value of the equivalent field for 
the *EM_CONTROL_CONTACT keyword. 
Contact Definition Cards.  Include one card for each contact definition.  This input ends at 
the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
Variable 
CONTID 
COTYPE 
PSIDM 
PSIDS 
EPS1 
EPS2 
EPS3 
8 
D0 
Type 
I 
Default 
none 
I 
0 
I 
I 
F 
F 
F 
F 
none 
none 
0.3 
0.3 
0.3 
None 
  VARIABLE   
DESCRIPTION
CONTID 
Electromagnetic contact ID 
COTYPE 
Type of EM contact  
EQ.0: Contact type 0 (Default).  
EQ.1: Contact type 1. 
PSIDM 
Master part set ID 
PSIDS 
EPSi 
Slave part set ID 
Contact  Coefficients  for  contact  detection  conditions.    See
discussion below. 
D0 
Contact condition 3 when COTYPE = 1. 
Remarks: 
Contact is detected when all of the following three condition are satisfied: 
1.  Contact condition 1: 
𝒏1. 𝒏2 ≤ −1 + 𝜀1
Figure 4-2.  Contact detection conditions between two faces. 
2.  Contact condition 2: 
−𝜺2 ≤ 𝛼1 ≤ 1 + 𝜀2 
−𝜺2 ≤ 𝛼2 ≤ 1 + 𝜀2 
−𝜺2 ≤ 𝛼3 ≤ 1 + 𝜀2  
With 𝑛1 and 𝑛2 the normal vectors of faces 𝑓1 and 𝑓2  respectfully and 𝑃 the projec-
tion of point 𝑎2 on face 𝑓1 with (𝛼1, 𝛼2, 𝛼3) its local coordinates . 
3.  Contact condition 3 depends on the contact type. 
a)  For contact type 0: 
𝑑 ≤ 𝜀3𝑆1 
where 𝑑 is the distance between 𝑃 and 𝑎2 and where 𝑆1 the minimum side 
length: 
𝑆1 = min[𝑑(𝑎1, 𝑏1), 𝑑(𝑏1, 𝑐1), 𝑑(𝑐1, 𝑎1)] 
b)  For contact type 1 : 
𝑑 ≤ 𝐷0
*EM_CONTACT_RESISTANCE 
Purpose:  Calculate the contact resistance of a previously defined EM contact in *EM_CON-
TACT.  Most contact resistance calculations are based on Ragmar Holm’s “Electric Contacts”. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CRID 
CONTID 
CTYPE 
CIRCID 
JHRTYPE
Type 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
Card 2 if CTYPE = 1. 
  Cards 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
Type 
I 
Default 
none 
Card 2 if CTYPE = 2. 
  Cards 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RHO 
RAD 
Type 
F 
Default 
0. 
F 
0.
Cards 2 
1 
2 
Variable 
RHO 
RAD 
Type 
F 
Default 
0. 
F 
0. 
Card 2 if CTYPE = 4. 
  Cards 2 
1 
2 
Variable 
RHO 
RAD 
Type 
F 
Default 
0. 
F 
0. 
Card 2 if CTYPE = 5. 
3 
D 
F 
0. 
3 
D 
F 
0. 
4 
5 
CURLCID 
EPS 
I 
0 
4 
CURLCID 
I 
0 
F 
0. 
5 
E 
F 
0. 
*EM 
7 
8 
6 
HB 
F 
0. 
6 
7 
8 
CURV 
F 
0. 
  Cards 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  RHOPROB  RHOSUB  RHOOXY 
FACTE 
FACFILM 
Type 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
CRID 
Resistive contact ID 
CONTID 
EM contact ID defined in *EM_CONTACT
VARIABLE   
DESCRIPTION 
CTYPE 
Contact Resistance type : 
EQ.1:  Contact resistance defined by user defined load curve. 
EQ.2:  Classic  Holm’s  formula  for  contact  resistances  . 
EQ.3:  Modified  contact  resistance  for  cases  with  plastic
deformation in the contact area . 
EQ.4:  Modified  contact  resistance  for  cases  with  elastic
deformation in the contact area . 
EQ.5:  Basic contact resistance definition . 
CIRCID 
Circuit ID: When defined, the contact resistance will be added to the
corresponding circuit total resistance and taken into account in the
circuit equations. 
JHRTYPE 
Indicates how the Joule heating calculated by the contact resistance 
shall be taken into account: 
EQ.0:  No addition: 
The  Joule  heating  calculated  by  the 
contact resistance is not taken into account. 
EQ.1:  The  Joule  heating  coming  from  the  contact  resistance  is
divided and distributed evenly among all elements neigh-
boring the contact surface. 
Load Curve ID defining the contact resistance versus time. 
Material resistivity ρmat.  If not defined or EQ.  0.0, the solver will 
automatically  calculate  an  average  resistivity  based  on  the
conductivity of the elements that are in contact. 
Radius of the contact sphere a.  If not defined or EQ.  0.0, the solver 
will  automatically  calculate  an  equivalent  radius  based  on  the
contact area:  𝑎 = √Area 𝜋⁄ . 
LCID 
RHO 
RAD 
D 
Diameter of the Electrode. 
CURLCID 
Load Curve ID defining the current intensity of the electrode.  If not
defined or EQ.  0, the solver will automatically look for the circuit’s
current intensity using the circuit defined in CIRID. 
EPS 
HB 
4-20 (EM) 
Constant 𝜀 with values typically between 0.35 and 1.
VARIABLE   
DESCRIPTION 
E 
Material Young’s modulus. 
CURV 
Radius of curvature of the contact surface, 𝑟. 
RHOPROB 
Probe resistivity, 𝜌prob 
RHOSUB 
Substrate resistivity, 𝜌sub 
RHOOXY 
Film resistivity, 𝜌oxi 
Scale  factor  on  the  constriction  area  when  calculating  the
constriction resistance.  If negative, the factor is time-dependent and 
defined by the load curve absolute value (FACTE). 
Scale  factor  on  the  constriction  area  when  calculating  the  film
resistance.  If negative, the factor is time-dependent and defined by 
the load curve absolute value (FACFILM). 
FACTE 
FACFILM 
Remarks: 
1.  Holm’s formula for Contact Resistance.  A very good approximation of the 
electric contact resistance is given by Holm’s formula : 
𝑅contact =
ρmat
2a
where ρmat is the material’s resistivity and a is the radius of the contact surface 
assuming the contact surface area is close to that of a circle : Area = 𝜋𝑎2.  
It is recommended to use this method (CTYPE = 2) in a first approach since most 
other contact resistance definitions are extensions of this formula. 
2.  Contact Area formulations.  For certain types of applications such as resistance 
spot welding (RSW) it is advantageous to better approximate the area by taking 
into account the deformation and the heterogeneities of the materials that come 
into contact at a microscopic level.  For a plastic deformation of the contact zone, 
the contact area, assumed to be circular, can be defined approximated as: 
Area =
𝐹𝑐
𝜀 𝐻𝑏
where 𝐹𝑐 is the contact force, 𝜀 a constant with values between 0.35 and 1, and 𝐻𝑏 
the Brinell hardness of the material. 
For an elastic deformation in the contact area, the radius of the contact surface is 
now given by:
2a
Current flow
Electrode
Lorentz  
Force: Fc
Curvature of the 
current lines induces 
a Lorentz Force
Contact Area
Workpiece
Figure  4-3.    Electrode  coming  into  contact  with  workpiece  (RSW
application). 
𝑎 =
1/3
𝑟𝐹𝑐
where 𝑟 is the radius of curvature of the contact surface and E is Young’s modulus. 
The Holm formula can then be modified in order to give: 
and 
𝑅contact =
ρmat
× √
𝜋𝜀𝐻𝑏
𝐹𝑐
𝑅contact =
ρmat
× (
𝑟𝐹𝑐
1/3
)
in the cases of plastic (CTYPE = 3) and elastic (CTYPE = 4) deformations respect-
fully. 
3.  Lorentz Force from a Spherical Electrode.  When a spherical electrode comes 
into contact with a work piece, the curvature of the current flowing from the elec-
trode to the work piece induces a Lorentz force parallel to the normal of the con-
tact surface thus forcing the electrode and the work piece away from each other.  
Its intensity can be written as: 
𝐹𝑐 =
𝜇0
4𝜋
𝐼2 ln (
2𝑎
)
where 𝐼 is the current intensity and 𝐷 the diameter of the electrode.  See Figure 4-3. 
4.  Basic resistive contact formulation (CTYPE = 5).  In the case of a clean metal 
contact with no film the resistance calculation involves only the constriction term.  
If a film is present and both sides have different metals, the contact resistance, 
𝑅contact, is the sum of the constriction resistance 𝑅constriction and the film resistance 
𝑅film.  In the basic resistive model, the following expressions determine the re-
sistance: 
𝑅constriction =
ρprob+ρsub
√FACTE × ContactArea
𝑅film =
𝜌oxy
√FACFILM × ContactArea
𝑅contact = 𝑅constriction + 𝑅film.
Purpose:  Enable the EM solver and set its options. 
*EM_CONTROL 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EMSOL 
NUMLS  MACRODT
Type 
Default 
I 
0 
I 
F 
100 
none 
  VARIABLE   
DESCRIPTION 
EMSOL 
Electromagnetism solver selector: 
EQ.1: Eddy current solver 
EQ.2: Induced heating solver 
EQ.3: Resistive heating solver 
NUMLS 
Number of local EM steps in a whole period for EMSOL = 2.  Not 
used for EMSOL = 1 
MACRODT 
Macro time step when EMSOL = 2.  Can be used as constant EM 
time  step  when  EMSOL = 1.    Obsolete:  use  *EM_CONTROL_-
TIMESTEP.
*EM 
Purpose:  This keyword activates the electromagnetism contact algorithms, which detects 
contact between conductors.  Electromagnetic fields to flow from one conductor to another 
when detected as in contact. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
Variable 
EMCT 
CCONLY 
COTYPE 
EPS1 
EPS2 
EPS3 
8 
D0 
Type 
Default 
I 
0 
I 
0 
I 
0 
F 
F 
F 
F 
0.3 
0.3 
0.3 
none 
  VARIABLE   
DESCRIPTION 
EMCT 
EM contact activation flag: 
EQ.0: No contact detection 
EQ.1: Contact detection 
CCONLY 
Determines on which parts of the model the EM contact should be 
activated. 
EQ.0: Contact detection between all active parts associated with a
conducting material.  (Default) 
EQ.1: Only look for EM contact between parts associated through
the  EM_CONTACT  card.    In  some  cases  this  option  can 
reduce the calculation time. 
COTYPE 
Type of EM contact.  If *EM_CONTACT is not defined, the solver 
will look for global contact options in *EM_CONTROL_CONTACT.
EQ.0: Contact type 0 (Default).  
EQ.1: Contact type 1. 
EPSi 
Global  contact  coefficients  used  if  the  equivalent  fields  in  *EM_-
CONTACT are empty. 
D0 
Global contact condition 3 value when COTYPE = 1
*EM_CONTROL_SWITCH 
Purpose:  It is possible to active a control “switch” that will shut down the solver based on 
a load curve information.  LS-DYNA incorporates complex types of curves  that allow the setting up of complex On/Off switches, for instance, by using a 
nodal temperature value. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
FEMCOMP  BEMCOMP
Type 
Default 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION 
LCID 
Load Curve ID.  
Negative values switch the solver off, positive values switch it back
on. 
FEMCOMP 
Determines  if  FEM  matrices  are  recomputed  each  time  the  EM
solver is turned back on : 
EQ.0 :  FEM matrices are recomputed 
EQ.1 :  FEM matrices are not recomputed 
BEMCOMP 
Determines  if  BEM  matrices  are  recomputed  each  time  the  EM
solver is turned back on : 
EQ.0 :  BEM matrices are recomputed 
EQ.1 :  BEM matrices are not recomputed
*EM 
Purpose:  It is possible to active a control “switch” that will shut down the electromagnetic 
contact detection.  This can be useful in order to save some calculation time in cases where 
the user knows when contact between conductors will occur or stop occurring. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCID 
NCYLFEM  NCYLFEM
Type 
Default 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION 
LCID 
Load Curve ID.  
Negative values switch the contact detection off, positive values
switch it back on. 
NCYLFEM 
NCYLBEM 
Determines the number of cycles before FEM matrix recomputation.
If defined this will overwrite the previous NCYCLFEM as long as the
contact detection is turned on. 
Determines the number of cycles before BEM matrix recomputa-
tion.  If defined this will overwrite the previous NCYCLBEM as long
as the contact detection is turned on.
Purpose:  Controls the EM time step and its evolution 
*EM_CONTROL_TIMESTEP 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TSTYPE  DTCONS 
LCID 
FACTOR 
Type 
I 
F 
I 
F 
Default 
none 
none 
none 
1.0 
  VARIABLE   
DESCRIPTION 
TSTYPE 
Time Step type 
EQ.1: constant time step given in DTCONST 
EQ.2: time step vs time given by a load curve specified in LCID
EQ.3: automatic time step computation, depending on the solver
type.  This time step is then multiplied by FACTOR 
DTCONST 
Constant value for the time step for TSTYPE = 1 
LCID 
Load curve ID giving the time step vs time for TSTYPE = 2 
FACTOR 
Multiplicative factor applied to the time step for TSTYPE = 3 
Remarks: 
1.  For an eddy current solver, the time step is based on the diffusion equation for the 
magnetic field.  
∂𝐴⃗
∂𝑡
+ ∇⃗⃗⃗⃗⃗ ×
∇⃗⃗⃗⃗⃗ × 𝐴⃗ + 𝜎∇⃗⃗⃗⃗⃗𝜑 = 𝚥 ⃗𝑆 
It is computed as the minimal elemental diffusion time step over the elements.  For 
a given element, the elemental diffusion time step is given as 𝑑𝑡𝑒 =
𝑙𝑒
⁄ , where: 
2𝐷
•  D is the diffusion coefficient 𝐷 = 1
⁄
𝜇0𝜎𝑒
, 
•  𝜎𝑒 is the element electrical conductivity,
•  𝜇0 is the permeability of free space, 
• 
𝑙𝑒 is the minimal edge length of the element (minimal size of the element).
*EM_DATABASE_CIRCUIT 
Purpose:  This keyword enables the output of EM data for every circuit defined.  
Output options card 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OUTLV 
DTOUT 
Type 
Default 
I 
1 
F 
0. 
  VARIABLE   
DESCRIPTION 
OUTLV 
Determines if the output file should be dumped. 
EQ.0: No output file is generated. 
EQ.1: The output file is generated. 
DTOUT 
Time interval to print the output.  If DTOUT is equal to 0.0, then the
EM timestep will be used. 
Remarks: 
1.  The file name for this database is em_circuit_XXX.dat with XXX the circuit ID. 
2.  ResistanceD is calculated in the following way: 
a)  A  scalar  potential  difference  of  1  is  imposed  at  the  circuit’s  boundaries 
SIDVIN and SIDVOUT. 
b)  The  system  to  be  solved  at  SIDCURR  is  then  ∇2𝜑 = 0  with  𝜑SIDVIN = 1 
and 𝜑SIDVOUT = 0.  No diffusive effects are taken into account meaning that 
the  current  density  can  be  written  as  𝐣 = ∇𝜑  and  the  total  current 
as 𝐼 = 𝐣 ⋅ 𝐧𝑑𝐴. 
c)  The resistance can then be estimated using 𝑅𝐷 = 𝑈 𝐼⁄ .  The calculation of 
this 𝑅𝐷 resistance is solely based on the circuit’s geometry and conductivi-
ty.  It is therefore equivalent to the resistance as commonly defined in the 
circuit equations: 
𝑅𝐷 = 𝐿 𝜎𝑆⁄
where L is the length of the circuit and S its surface area. 
3.  ResistanceJ  is  calculated  by  using  the  data  provided  during  the  EM  solve  : 
𝑅𝐽 = 𝐽 𝐼2⁄  where J and I are, respectively, the joule heating and the current.  Com-
pared with ResistanceD, ResistanceJ is not so much a resistance calculation since 
it accounts for the resistive effects (when using the Eddy current solver).  Rather, it 
corresponds to the resistance that the circuit would need in order to get the same 
Joule heating in the context of a circuit equation.  If all EM fields are diffused or the 
RH solver is being used, ResistanceJ should be close to ResistanceD. 
4.  Only the mutual inductances between the first three circuits defined are output.
*EM_DATABASE_CIRCUIT0D 
Purpose:  This keyword enables the output of EM data for every circuit defined.  
Output options card 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OUTLV 
DTOUT 
Type 
Default 
I 
0 
F 
0. 
  VARIABLE   
DESCRIPTION 
OUTLV 
Determines if the output file should be dumped. 
EQ.0:  No output file is generated. 
EQ.1:  The output file is generated. 
DTOUT 
Time interval to print the output.  If DTOUT is equal to 0.0, then the
EM timestep will be used. 
Remarks: 
1.  The file name for this database is em_circuit0D_XXX.dat with XXX the circuit ID.  
2.  At the start of the run, based on the initial values of the meshes resistances and 
inductances,  the  solver  will  calculate  the  results  for  a  so-called  “0D”  solution 
which does not take into account the current’s diffusion, the part’s displacements 
or the EM material property changes.  It is therefore a crude approximation.  This 
can be useful in some cases especially in R,L,C circuits if the users wishes to have 
an first idea of how the source current will behave. 
3.  Since the calculation of this 0D circuit can take time depending on the problems 
size, it should only be used in cases where the output results are useful to the 
comprehension of  the analysis. 
4.  This card has no influence on the results of the EM run itself.
*EM 
Purpose:  This keyword enables the output of EM data on elements.  
Output Options Card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OUTLV 
DTOUT 
Type 
Default 
I 
0 
F 
0. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ELSID 
Type 
I 
Default 
none 
  VARIABLE   
DESCRIPTION 
OUTLV 
Determines if the output file should be dumped. 
EQ.0:  No output file is generated. 
EQ.1:  The output file is generated. 
DTOUT 
Time interval to print the output.  If DTOUT is equal to 0.0, then the
EM timestep will be used. 
ELSID 
Solid Elements Set ID. 
Remarks: 
1.  The file name for this database is em_elout.dat.
*EM_DATABASE_FIELDLINE 
Purpose:    The  EM  solver  uses  a  BEM  method  to  calculate  the  EM  fields  between 
conductors.  With this method, the magnetic field in the air or vacuum between conductors 
is therefore not explicitly computed.  However, in some cases, it may be interesting to 
visualize some magnetic field lines for a better analysis.  This keyword allows the output of 
field line data.  It has no influence on the results of the EM solve. 
Output Options Card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FLID 
PSID 
DTOUT 
NPOINT 
Type 
I 
I 
F 
I 
Default 
none 
none 
0. 
100 
Remaining cards are optional.† 
  Card 2 
1 
Variable 
INTEG 
Type 
Default 
I 
2 
2 
H 
F 
3 
4 
5 
6 
7 
8 
HMIN 
HMAX 
TOLABS 
TOLREL 
F 
F 
F 
F 
0. 
0. 
1E10 
1E-3 
1E-5 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
BTYPE 
Type 
Default 
I
VARIABLE   
DESCRIPTION 
FLID 
PSID 
Field line set ID 
Point Set ID associated to the field line set . 
The coordinates given by the different points will be the starting
points of the field lines. 
DTOUT 
Time interval to print the output.  If DTOUT is equal to 0.0, then the
EM time step will be used. 
NPOINT 
Number of points per field line.  The points are regularly spaced. 
INTEG 
Type of numerical integrator used to compute the field lines : 
EQ.1: RK4, Runge Kutta 4.  See Remark 2. 
EQ.2: DOP853, Dormand Prince 8(5,3).  See Remark 2. 
Value of the step size.  In case of an integrator with adaptive step
size, it is the initial value of the step size. 
Minimal step size value.  Only used in the case of an integrator with
adaptive step size. 
Maximal step size value.  Only used in the case of an integrator with
adaptive step size. 
Absolute tolerance of the integrator.  Only used in the case of an 
integrator with adaptive step size. 
Relative  tolerance  of  the  integrator.    Only  used  in  the  case  of  an
integrator with adaptive step size. 
H 
HMIN 
HMAX 
TOLABS 
TOLREL 
BTYPE 
Method to compute the magnetic field : 
EQ.1: Direct method (every contribution is computed by the Biot 
Savart Law and summed up : very slow). 
EQ.2: Multipole  method  (approximation  of  the  direct  method
using the multipole expansion). 
EQ.3: Multicenter method (approximation of the direct method
using a weighted subset of points only in order to compute
the magnetic field).
*EM_DATABASE_FIELDLINE 
1.  File Names.  The file name for this database is em_fieldLine_XX_YYY.dat where XX 
is the field line ID and YYY is the point set ID defined in *EM_POINT_SET. 
2. 
Integrators.    The  Runge  Kutta  4  integrator  is  an  explicit  iterative  method  for 
solving ODEs.  It is a fourth order method with a constant step size.  The Dormand 
Prince 8(5,3) integrator is an explicit iterative method for solving IDEs.  Particular-
ly, this integrator is an embedded Runge Kutta integrator of order 8 with an adap-
tive step size.  This integrator allows a step size control which is done though an 
error estimate at each step.  The Dormand Prince 8(5,3) is a Dormand Prince 8(6) 
for which the 6th order error estimator has been replaced by a 5th order estimator 
with 3rd order correction in order to make the integrator more robust.
Purpose:  This keyword enables the output of global EM. 
Output Options Card. 
*EM 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OUTLV 
DTOUT 
Type 
Default 
I 
0 
F 
0. 
  VARIABLE   
DESCRIPTION 
OUTLV 
Determines if the output file should be dumped. 
EQ.0:  No output file is generated. 
EQ.1:  The output file is generated. 
DTOUT 
Time interval to print the output.  If DTOUT is equal to 0.0, then the
EM timestep will be used. 
Remarks: 
1.  The file name for this database is em_globEnergy.dat.  
2.  Outputs the global EM energies of the mesh, the air and the source circuit.  Also 
outputs the global kinetic energy and the global plastic work energy.
*EM_DATABASE_NODOUT 
Purpose:  This keyword enables the output of EM data on nodes.  
Output Options Card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OUTLV 
DTOUT 
Type 
Default 
I 
0 
F 
0. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NSID 
Type 
I 
Default 
none 
  VARIABLE   
DESCRIPTION 
OUTLV 
Determines if the output file should be dumped. 
EQ.0:  No output file is generated. 
EQ.1:  The output file is generated. 
DTOUT 
Time interval to print the output.  If DTOUT is equal to 0.0, then the
EM timestep will be used. 
NSID 
Node Set ID. 
Remarks: 
1.  The file name for this database is em_nodout.dat.
*EM 
Purpose:  This keyword enables the output of EM data for every part defined.  . 
Output Options Card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OUTLV 
DTOUT 
Type 
Default 
I 
0 
F 
0. 
  VARIABLE   
DESCRIPTION 
OUTLV 
Determines if the output file should be dumped. 
EQ.0:  No output file is generated. 
EQ.1:  The output file is generated. 
DTOUT 
Time interval to print the output.  If DTOUT is equal to 0.0, then the
EM timestep will be used. 
Remarks: 
1.  The file name for this database is em_partData_XXX.dat with XXX the part ID.  
2.  Outputs the part EM energies of the part as well as the Lorentz force.  Also outputs 
the part kinetic energy and the part plastic work energy.
*EM_DATABASE_POINTOUT 
Purpose:  This keyword enables the output of EM data on points sets.  
Output Options Card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OUTLV 
DTOUT 
Type 
Default 
I 
0 
F 
0. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PSID 
Type 
I 
Default 
none 
  VARIABLE   
DESCRIPTION 
OUTLV 
Determines if the output file should be dumped. 
EQ.0: No output file is generated. 
EQ.1: The output file is generated. 
DTOUT 
Time interval to print the output.  If DTOUT is equal to 0.0, then the
ICFD timestep will be used. 
PSID 
Point Set ID . 
Remarks: 
1.  The file name for this database is em_pointout.dat.
*EM 
Purpose:  This keyword enables the output of EM data for every circuit defined.  . 
Output Options Card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OUTLV 
DTOUT 
Type 
Default 
I 
1 
F 
0. 
  VARIABLE   
DESCRIPTION 
OUTLV 
Determines if the output file should be dumped. 
EQ.0:  No output file is generated. 
EQ.1:  The output file is generated. 
DTOUT 
Time interval to print the output.  If DTOUT is equal to 0.0, then the
EM timestep will be used. 
Remarks: 
1.  The file name for this database is em_rogoCoil_XXX.dat  where XXX is the rogo 
Coil ID.
*EM_DATABASE_TIMESTEP 
Purpose:  This keyword enables the output of EM data regarding the EM timestep. 
Output options card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OUTLV 
Type 
Default 
I 
0 
  VARIABLE   
DESCRIPTION 
OUTLV 
Determines if the output file should be dumped. 
EQ.0:  No output file is generated. 
EQ.1:  The output file is generated. 
Remarks: 
1.  The file name for this database is em_timestep.dat.  
2.  Outputs the run’s EM tim estep versus the time step calculated using the EM CFL 
condition as criteria (autotimestep).  This can be useful in cases with big defor-
mations and/or material property changes and a fixed time step is being used in 
case that time step becomes to big compared to the stability time step.
*EM 
Purpose:  Define the parameters for a Burgess model giving the electrical conductivity as 
as a function of the temperature and the density, see: 
T.J.  Burgess, “Electrical resistivity model of metals”, 4th International Conference on Megagauss 
Magnetic-Field Generation and Related Topics, Santa Fe, NM, USA, 1986 
  Card 1 
1 
Variable 
EOSID 
Type 
I 
2 
V0 
F 
3 
4 
GAMMA 
THETA 
F 
F 
5 
LF 
F 
6 
C1 
F 
7 
C2 
F 
8 
C3 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 2 
Variable 
1 
C4 
Type 
F 
2 
K 
F 
3 
4 
5 
6 
7 
8 
EXPON 
LGTUNIT  TIMUNIT 
TEMUNI 
ADJUST 
I 
F 
F 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
In the following, UUS stands for User Units System and BUS for Burgess Units  
  VARIABLE   
DESCRIPTION 
EOSID 
ID of the EM_EOS (specified by an *EM_MAT card) 
V0 
Reference specific volume V0 (UUS). 
GAMMA0 
Reference Gruneisen value γ0.(no units). 
THETA 
Reference melting temperature θm,0 in eV (BUS). 
LF 
C1 
C2 
Latent heat of fusion LF in kJoule/mol (BUS). 
C1 constant (BUS) 
C2 constant (no units)
VARIABLE   
DESCRIPTION 
C3 
C4 
K 
C3 constant (no units) 
C4 constant (no units) 
Parameter k (no units). 
EXPON 
Exponent in equations (2)  
LGTUNIT 
Length units for UUS (relative to meter, i.e. = 1.e-3 if UUS in mm).
TIMUNIT 
Time units for UUS (relative to seconds). 
TEMUNIT 
Temperature units 
EQ.1: temperature in Celsius 
EQ.2: temperature in Kelvins 
ADJUST 
Conductivity modification 
EQ.0: (default) The conductivity is given by the Burgess formula.
EQ.1: The  conductivity  is  adjusted  so  that  it  is  equal  to  the
conductivity defined in *EM_MAT card σmat at room tem-
perature: 
σ(θ) = σBurgess(θ)
σmat
σBurgess(θroom)
Remarks: 
1.  The Burgess model gives the electrical resistivity vs temperature and density for 
the solid phase, liquid phase and vapor phase.  At this time, only the solid and 
liquid phases are implemented.  To check which elements are in the solid and in 
the liquid phase, a melting temperature is first computed by: 
θ𝑚 = θ𝑚,0 (
𝑉0
−1
)
(2γ0−1)(1− 𝑉
𝑉0
)
If T < 𝜃𝑚: solid phase model applies. 
a) 
The solid phase electrical resistivity corresponds to the Meadon model: 
η𝑆 = (𝐶1 + 𝐶2θ𝐶3)𝑓𝑐 (
𝑉0
),
(1)
where θ is the temperature, V is the specific volume, and V0 is the reference 
specific volume (zero pressure, solid phase).  In (1), the volume dependence 
is given by:
2γ−1
2γ+1
2γ
)
)
)
EXPON.EQ. −1 
(most materials)
EXPON.EQ. +1 
(tungsten)
EXPON.EQ. 0
(stainless steel)
(
(
(
𝑉0
𝑉0
𝑉0
⎧
{
{
{
{
{
⎨
{
{
{
{
{
⎩
𝑓𝑐 (
𝑉0
) =
with 
γ = γ0 − (γ0 −
) (1 −
𝑉0
)
b) 
If T > θm : liquid phase model: 
η𝐿 = (η𝐿)θ𝑚 (
θ𝑚
𝐶4
)
(η𝐿)θ𝑚 = Δη(η𝑆)θ𝑚 
with 
where 
(2)
(3)
(4)
Δ𝜂 =
⎧𝑘𝑒0.69𝐿𝐹/θ𝑚
{{
⎨
{{
⎩
1 + 0.0772(2 − θ𝑚)
1 + 0.106(0.846 − θ𝑚)
𝑘 > 0
𝑘 = −1
(tungsten)
(5)
𝑘 = −2
(stainless steel SS-304)
The following table reports some sets of parameters given by Burgess in his 
paper: 
Parameter 
Cu 
Ag 
Au 
W 
Al(2024) 
SS(304) 
V0(cm3/gm) 
0.112 
0.0953 
0.0518 
0.0518 
0.370 
0.1265 
γ0 
θm,0 (BUS) 
2.00 
2.55 
3.29 
1.55 
2.13 
2.00 
0.117 
0.106 
0.115 
0.315 
0.0804 
0.156 
LF (BUS) 
0.130 
0.113 
0.127 
0.337 
0.107 
0.153 
C1 (BUS) 
-4.12e-5 
-3.37e-5 
-4.95e-5 
-9.73e-5 
-5.35e-5 
0 
C2 
C3 
0.113 
0.131 
0.170 
0.465 
0.233 
0.330 
1.145 
1.191 
1.178 
1.226 
1.210 
0.4133 
EXPON 
-1 
-1 
-1 
+1 
-1
Parameter 
Cu 
Ag 
Au 
W 
Al(2024) 
SS(304) 
C4 
k 
0.700 
0.672 
0.673 
0.670 
0.638 
0.089 
0.964 
0.910 
1.08 
-1. 
0.878 
-2.
*EM 
Purpose:  Define the parameters for a Meadon model, giving the electrical conductivity as a 
function of the temperature and the density; see: 
T.J.  Burgess, “Electrical resistivity model of metals”, 4th International Conference on Megagauss 
Magnetic-Field Generation and Related Topics, Santa Fe, NM, USA, 1986 
  Card 1 
1 
Variable 
EOSID 
Type 
I 
2 
C1 
F 
3 
C2 
F 
4 
C3 
F 
5 
TEMUNI 
I 
6 
V0 
F 
7 
8 
GAMMA 
EXPON 
F 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LGTUNIT  TIMUNIT 
ADJUST 
Type 
F 
F 
I 
Default 
none 
none 
none 
In the following, UUS stands for User Units System and BUS for Burgess Units. 
  VARIABLE   
DESCRIPTION 
EOSID 
ID of the EM_EOS 
C1 
C2 
C3 
C1 constant (BUS) 
C2 constant (no units) 
C3 constant (no units) 
TEMUNIT 
Temperature units 
EQ.1: temperature in Celsius 
EQ.2: temperature in Kelvins
VARIABLE   
DESCRIPTION 
V0 
Reference specific volume V0 (UUS). 
GAMMA0 
Reference Gruneisen value γ0.(no units). 
EXPON 
Exponent in equations (7) 
LGTUNIT 
Length units for UUS (relative to meter, i.e. = 1.e-3 if UUS in mm).
TIMUNIT 
Time units for UUS (relative to seconds). 
ADJUST: 
EQ.0: (default) the conductivity is given by the Burgess formula.
EQ.1: The  conductivity  is  adjusted  so  that  it  is  equal  to  the
conductivity defined in the *EM_MAT card σmatat room 
temperature: 
σ(θ) = σBurgess(θ)
σmat
σBurgess(θroom)
Remarks: 
1.  The Meadon model is a simplified Burgess model with the solid phase equations 
only. 
The electrical resistivity is given by: 
η𝑆 = (𝐶1 + 𝐶2θ𝐶3)𝑓𝑐 (
𝑉0
) 
(6)
where θ is the temperature, V is the specific volume, and V0 is the reference specif-
ic volume (zero pressure, solid phase). 
In (6), the volume dependence is given by: 
𝑓𝑐 (
𝑉0
) =
⎧
{
{
{
{
{
{
⎨
{
{
{
{
{
{
⎩
2γ−1
2γ+1
2γ
)
)
)
EXPON.EQ. −1
(most materials)
EXPON.EQ. +1
(tungsten)
(7)
EXPON.EQ.0
(stainless steel)
(
(
(
𝑉0
𝑉0
𝑉0
VO.EQ. 0
(default value for 𝑉0 is zero)
 (In this last case, only EOSID, C1, C2, C3, TEMUNIT, TIMUNIT and LGTUNIT 
need to be defined) 
with,
) (1 −
𝑉0
) 
*EM 
(8)
The following table reports some sets of parameters given by Burgess in his paper: 
Parameter 
Cu 
Ag 
Au 
W 
Al(2024) 
SS(304) 
V0(cm3/gm) 
0.112 
0.0953 
0.0518 
0.0518 
0.370 
0.1265 
γ0 
2.00 
2.55 
3.29 
1.55 
2.13 
2.00 
C1 (BUS) 
-4.12e-5 
-3.37e-5 
-4.95e-5 
-9.73e-5 
-5.35e-5 
0 
C2 
C3 
0.113 
0.131 
0.170 
0.465 
0.233 
0.330 
1.145 
1.191 
1.178 
1.226 
1.210 
0.4133 
EXPON 
-1 
-1 
-1 
+1 
-1
*EM_EOS_PERMEABILITY 
Purpose:  Define the parameters for the behavior of a material’s permeability 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EOSID 
EOSTYPE 
LCID 
Type 
I 
I 
I 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
EOSID 
ID of the EM_EOS 
EOSTYPE 
Define the type of EOS: 
EQ.1: Permeability defined by a B function of H curve (B = µH)
EQ.2: Permeability defined by a H function of B curve (H = B/µ)
LCID 
Load curve ID
*EM 
Purpose:  Define the electrical conductivity as a function of temperature by using a load 
curve. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EOSID 
LCID 
Type 
I 
I 
Default 
none 
none 
  VARIABLE   
DESCRIPTION 
EOSID 
ID of the EM_EOS 
LCID 
Load curve ID. 
Remarks: 
1.  The load curve describes the electrical conductivity (ordinate) vs the temperature 
(abscissa).  The user needs to make sure the temperature and the electrical conduc-
tivity given by the load curve are in the correct units.  Also, it is advised to give 
some bounds to the load curve (conductivities at very low and very high tempera-
tures) to avoid bad extrapolations of the conductivity if the temperature gets out of 
the load curve bounds.
*EM_EOS_TABULATED1 
Purpose:  Define the electrical conductivity as a function of time by using a load curve. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
EOSID 
LCID 
Type 
I 
I 
Default 
none 
none 
  VARIABLE   
DESCRIPTION 
EOSID 
ID of the EM_EOS 
LCID 
Load curve ID. 
Remarks: 
1.  The  load  curve  describes  the  electrical  conductivity  (ordinate)  vs  the  time 
(abscissa).  The user needs to make sure the time and the electrical conductivity 
given by the load curve are in the correct units.  Also, it is advised to give some 
bounds to the load curve (conductivities at t = 0 at after a long time) to avoid bad 
extrapolations of the conductivity if the run time gets out of the load curve bounds. 
2.  LCID can also refer to a DEFINE FUNCTION.  If a DEFINE_FUNCTION is used, 
allowed: 
the 
 𝑓 (𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑣𝑜𝑙, 𝑚𝑎𝑠𝑠, 𝐸𝑥, 𝐸𝑦, 𝐸𝑧, 𝐵𝑥, 𝐵𝑦, 𝐵𝑧, 𝐹𝑥, 𝐹𝑦, 𝐹𝑧, 𝐽𝐻𝑟𝑎𝑡𝑒, 𝑡𝑖𝑚𝑒). 
𝐹𝑥, 𝐹𝑦, 𝐹𝑧  refers to the Lorentz force vector.
parameters 
following 
are
*EM 
Purpose:    Define  the  components  of  a  time  dependent  exterior  field  uniform  in  space 
applied on the conducting parts. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
FIELDID 
FTYPE 
FDEF 
LCIDX 
LCIDY 
LCIDZ 
Type 
Default 
I 
0 
I 
0 
F 
0 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION 
FIELDID 
External Field ID 
FTYPE 
Field type:  
EQ.1: Magnetic field 
EQ.2: Electric field (not available yet) 
FDEF 
Field defined by : 
EQ.1: Load Curves 
LCID[X,Y,Z] 
Load curve ID defining the (X,Y,Z) component of the field function 
of time
*EM_EXTERNAL_FIELD 
Purpose:  Defining an isopotential, i.e.  constrain nodes so that they have the same scalar 
potential value.  This card is to be used with the EM solver of type 3 and the distributed 
Randle circuits only at this time. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ISOID 
SETTYPE 
SETID 
Type 
I 
I 
I 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
ISOID 
ID of the Isopotential 
SETTYPE 
Set type: 
EQ.2: Node Set. 
SETID 
Set ID
Purpose: Define a connection between two isopotentials. 
*EM 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CONID 
CONTYPE 
ISOID1 
ISOID2 
VAL 
LCID 
Type 
I 
I 
I 
I 
F 
I 
Default 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
CONID 
Connection ID 
CONTYPE 
Connection type : 
EQ.1: Short Circuit. 
EQ.2: Resistance. 
EQ.3: Voltage Source. 
EQ.4: Current Source. 
ISOID1 
ID of the first isopotential to be connected 
ISOID2 
ID of the second isopotential to be connected 
VAL 
LCID 
Value of the resistance, voltage or current depending on CONTYPE
Ignored if LCID defined. 
Load  curve  ID  defining  the  value  of  the  resistance,  voltage  or
current  function  of  time  and  depending  on  CONTYPE.    If  not 
defined, VAL will be used.
*EM_MAT_001 
Purpose:  Define the electromagnetic material type and properties for a material whose 
permeability equals the free space permeability. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
MTYPE 
SIGMA 
EOSID 
Type 
I 
I 
F 
I 
Default 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
MID 
Material ID: refers to MID in the *PART card. 
MTYPE 
Defines the electromagnetism type of the material: 
EQ.0: Air or vacuum 
EQ.1: Insulator  material. 
  these  materials  have  the  same
electromagnetism behavior as EQ.0 
EQ.2: Conductor  carrying  a  source.    In  these  conductors,  the
eddy  current  problem  is  solved,  which  gives  the  actual
current density.  Typically, this would correspond to the 
coil. 
EQ.4: Conductor not connected to any current or voltage source,
where the Eddy current problem is solved.  Typically, this
would correspond to the workpiece 
SIGMA 
Initial electrical conductivity of the material 
EOSID 
ID of the EOS to be used for the electrical conductivity .
*EM 
Purpose:  Define an electromagnetic material type and properties whose permeability is 
different than the free space permeability. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
MTYPE 
SIGMA 
EOSID 
MUREL 
EOSMU 
Type 
I 
I 
F 
I 
F 
I 
Default 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
MID 
Material ID: refers to MID in the *PART card. 
MTYPE 
Defines the electromagnetism type of the material: 
EQ.0: Air or vacuum 
EQ.1: Insulator  material.    These  materials  have  the  same
electromagnetism behavior as EQ.0 
EQ.2: Conductor  carrying  a  source.    In  these  conductors,  the
eddy  current  problem  is  solved,  which  gives  the  actual
current density.  Typically, this would correspond to the 
coil. 
EQ.4: Conductor not connected to any current or voltage source,
where the Eddy current problem is solved.  Typically, this
would correspond to the workpiece 
SIGMA 
Initial electrical conductivity of the material 
EOSID 
MUREL 
EOSMU 
ID of the EOS to be used for the electrical conductivity . 
Relative permeability: Is the ratio of the permeability of a specific
medium to the permeability of free space (𝜇𝑟 = 𝜇/𝜇0) 
ID of the EOS to be used to define the behavior of µ by an equation 
of state (Note: if EOSMU is defined, MUREL will be used for the
initial value only).
*EM_MAT_002 
Purpose:  Define an electromagnetic material type whose electromagnetic conductivity is 
defined by a (3*3) tensor matrix.  Applications include composite materials. 
Orthotropic Card 1.   
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
MTYPE 
SIGMA11 SIGMA22 SIGMA33
Type 
I 
I 
F 
F 
F 
Orthotropic Card 2.   
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  SIGMA12  SIGMA13  SIGMA21 SIGMA23 SIGMA31 SIGMA32 
AOPT 
Type 
F 
F 
F 
F 
F 
F 
I 
Orthotropic Card 3.   
  Card 1 
Variable 
1 
XP 
Type 
F 
Orthotropic Card 4.   
  Card 2 
Variable 
1 
V1 
Type 
F 
2 
YP 
F 
2 
V2 
F 
7 
8 
MACF 
I 
7 
8 
3 
ZP 
F 
3 
V3 
F 
4 
A1 
F 
4 
D1 
5 
A2 
F 
5 
D2 
6 
A3 
F 
6 
D3 
F 
F 
F 
  VARIABLE   
DESCRIPTION 
MID 
Material ID: refers to MID in the *PART card.
MTYPE 
Defines the electromagnetism type of the material: 
EQ.0: Air or vacuum 
EQ.1: Insulator material: These  materials  have 
electromagnetism behavior as EQ.0 
the 
same 
EQ.2: Conductor carrying a source.  In these conductors, the eddy
current problem is solved, which gives the actual current
density.  Typically, this would correspond to the coil. 
EQ.4: Conductor not connected to any current or voltage source, 
where the Eddy current problem is solved.  Typically, this
would correspond to the workpiece. 
SIGMA11 
SIGMA12 
The  1,  1  term  in  the  3  ×  3  electromagnetic  conductivity  tensor 
matrix.  Note that 1 corresponds to the a material direction 
The  1,  2  term  in  the  3  ×  3  electromagnetic  conductivity  tensor 
matrix.  Note that 2 corresponds to the b material direction 
⋮ 
⋮  
SIGMA33 
The  3,  3  term  in  the  3  ×  3  electromagnetic  conductivity  tensor 
matrix. 
Define AOPT for both options: 
AOPT 
Material axes option, see the figure in *MAT_002. 
EQ.0.0:  locally  orthotropic  with  material  axes  determined  by
element  nodes  as  shown  in  part  (a)  the  figure  in
*MAT_002.  The a-direction is from node 1 to node 2 of 
the  element.    The  b-direction  is  orthogonal  to  the  a-
direction and is in the plane formed by nodes 1, 2, and 4.
EQ.1.0:  locally orthotropic with material axes determined by a
point in space and the global location of the element cen-
ter; this is the a-direction.   
EQ.2.0:  globally orthotropic with material axes determined by 
vectors  defined  below,  as  with  *DEFINE_COORDI-
NATE_VECTOR. 
EQ.3.0:  locally orthotropic material axes determined by rotating
the material axes about the element normal by an angle,
BETA, from a line in the plane of the element defined by 
the cross product of the vector v with the element nor-
mal.  The plane of a solid element is the midsurface be-
tween the inner surface and outer surface defined by the
first four nodes and the last four nodes of the connectivi-
ty of the element, respectively. 
EQ.4.0:  locally orthotropic in cylindrical coordinate system with
the material axes determined by a vector v, and an origi-
nating point, P, which define the centerline axis.  This op-
tion is for solid elements only. 
EQ.5.0:  globally defined reference frame with (a,b,c)=(X0,Y0,Z0).
XP, YP, ZP 
Define coordinates of point p for AOPT = 1 and 4. 
A1, A2, A3 
Define components of vector a for AOPT = 2. 
MACF 
Material axes change flag for solid elements: 
EQ.1:  No change, default, 
V1, V2, V3 
Define components of vector v for AOPT = 3 and 4. 
D1, D2, D3 
Define components of vector d for AOPT = 2. 
Remarks: 
This card works in a similar way to *MAT_002. 
The  procedure  for  describing  the  principle  material  directions  is  explained  for  solid 
elements for this material model.  We will call the material direction the a-b-c coordinate 
system.  The AOPT options illustrated in the AOPT figure of *MAT_002 can define the a-b-
c system for all elements of the parts that use the material.
*EM 
Purpose:  Define the electromagnetic material type and properties for conducting shells in a 
3D problem. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MID 
MTYPE 
SIGMA 
EOSID 
NELE 
Type 
I 
I 
F 
I 
Default 
none 
none 
none 
none 
I 
1 
  VARIABLE   
DESCRIPTION 
MID 
Material ID: refers to MID in the *PART card. 
MTYPE 
Defines the electromagnetism type of the material: 
EQ.0: Air or vacuum 
EQ.1: Insulator  material. 
  these  materials  have  the  same
electromagnetism behavior as EQ.0 
EQ.2: Conductor  carrying  a  source.    In  these  conductors,  the
eddy  current  problem  is  solved,  which  gives  the  actual
current density.  Typically, this would correspond to the 
coil. 
EQ.4: Conductor not connected to any current or voltage source,
where the Eddy current problem is solved.  Typically, this
would correspond to the workpiece 
SIGMA 
Initial electrical conductivity of the material 
EOSID 
NELE 
ID of the EOS to be used for the electrical conductivity . 
Number of elements in the thickness of the shell.  It is up to the user
to  make  sure  his  mesh  is  fine  enough  to  correctly  capture  the
inductive-diffusive effects .
*EM_OUTPUT 
Purpose:  Define the level of EM related output on the screen and in the messag file. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MATS 
MATF 
SOLS 
SOLF 
MESH 
MEM 
TIMING 
Type 
Default 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION 
MATS 
Level of matrix assembly output to the screen: 
EQ.0: No output 
EQ.1: Basic assembly steps 
EQ.2: Basic assembly steps+percentage completed+final statistics
EQ.3: Basic  assembly  steps+percentage  completed+statistics  at
each percentage of completion 
MATF 
Level of matrix assembly output to the messag file: 
EQ.0: No output 
EQ.1: Basic assembly steps 
EQ.2: Basic assembly steps+percentage completed+final statistics
EQ.3: Basic  assembly  steps+percentage  completed+statistics  at
each percentage of completion 
SOLS 
Level of solver output on the screen: 
EQ.0: No output 
EQ.1: Global information at each FEM iteration 
EQ.2: Detailed information at each FEM iteration
DESCRIPTION 
*EM 
SOLF 
Level of solver output to the messag file: 
EQ.0: No output 
EQ.1: Global information at each FEM iteration 
EQ.2: Detailed information at each FEM iteration 
MESH 
Controls the output of the mesh data to the d3hsp file 
EQ.0: No mesh output 
EQ.1: Mesh info is written to the d3hsp file 
MEMORY 
Controls the output of information about the memory used by the 
EM solve to the messag file: 
EQ.0: no memory information written. 
EQ.1: memory information written. 
TIMING 
Controls  the  output  of  information  about  the  time  spent  in  the
different parts of the EM solver to the messag file 
EQ.0: no timing information written. 
EQ.1: timing information written.
*EM_OUTPUT 
Purpose:  This keyword creates a set of points which  can be used  by the *EM_DATA-
BASE_POINTOUT keyword.  
Output Options Card. 
  Card 1 
1 
2 
Variable 
PSID 
PSTYPE 
Type 
Default 
I 
0 
I 
0 
3 
VX 
F 
0. 
4 
VY 
F 
0. 
5 
VZ 
F 
0. 
6 
7 
8 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
5 
6 
7 
8 
  Card 2 
1 
Variable 
PID 
Type 
I 
2 
X 
F 
3 
Y 
F 
4 
Z 
F 
Default 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
PSID 
Point Set ID. 
PSTYPE 
Point Set type : 
EQ.0: Fixed points. 
EQ.1: Tracer points using prescribed velocity. 
VX, VY, VZ 
Constant velocities to be used when PSTYPE = 1 
PID 
Point ID 
X, Y, Z 
Point initial coordinates
*EM 
Purpose: For battery cell internal short, define conditions to turn on a Randle short (replace 
one or several randle circuits by resistances), and to define the value of the short resistance. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  AREATYPE  FUNCID 
Type 
I 
I 
Default 
none 
none 
  VARIABLE   
DESCRIPTION 
AREATYPE 
Works the same way as RDLAREA in *EM_CIRCUIT_RANDLE : 
EQ.0: The  resistance  in  FUNCTIONID  is  taken  as  is  in  each 
Randle circuit. 
EQ.1:  The resistance in FUNCTIONID is per unit area. 
EQ.2: The resistance in FUNCTIONID is  for the whole unit cell
(the whole cell is shorted), and then a factor based on ar-
eaLocal/areaGlobal is applied. 
FUNCTIONID 
DEFINE_FUNCTION ID giving the local resistance function of local
parameters  for  the  local  randle  circuit.    Accepted  values  are:
 𝑓 (𝑥𝑐𝑐𝑝, 𝑦𝑐𝑐𝑝, 𝑧𝑐𝑐𝑝, 𝑥𝑠𝑒𝑝, 𝑦𝑠𝑒𝑝, 𝑧𝑠𝑒𝑝, 𝑥𝑠𝑒𝑚, 𝑦𝑠𝑒𝑚, 𝑧𝑠𝑒𝑚, 𝑥𝑐𝑐𝑚, 𝑦𝑐𝑐𝑚, 𝑧𝑐𝑐𝑚, 𝑡𝑖𝑚𝑒).  
Remarks: 
1. 
If the return value of the function is negative, there is no short, the randle circuit is 
maintained.  If it is negative, the function gives the value of the reistance. 
2.  The parameter description is : 
a) 
x_ccp: x of boundary between positive current collector and positive elec-
trode 
b)  x_sep: x of boundary between positive electrode and separator
c) 
x_sem: x of boundary between separator and negative electrode 
d)  x_ccm: x of boundary between negative electrode and negative current col-
lector 
3.  An example of a function :  
*DEFINE_FUNCTION 
FID (Function Id) 
Float resistance_short_randle( 
float time, 
 float x_ccp,float y_ccp,float z_ccp, 
float x_sep,float y_sep,float z_sep, 
float x_sem,float y_sem,float z_sem, 
float x_ccm,float y_ccm,float z_ccm) 
{ float seThick0; 
seThick0 = 1.e-5; 
   seThick=(sqrt(x_sep-x_sem)^2+(y_sep-y_sem)^2+(z_sep-z_sem)^2); 
if (seThick >= seThick0) then 
return -1; 
else 
return 1.e-2; 
endif
*EM 
Purpose:  Define a rotation axis for the EM solver.  This is used with the 2D axisymmetric 
solver.  The axis is defined by a point and a direction. 
  Card 1 
Variable 
1 
XP 
Type 
F 
2 
YP 
F 
3 
ZP 
F 
4 
XD 
F 
5 
YD 
F 
6 
7 
8 
ZD 
NUMSEC 
F 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
XP, YP, ZP 
𝑥, 𝑦, and 𝑧 coordinates of the point 
XD, YD, ZD 
𝑥, 𝑦, and 𝑧 components of direction of the axis 
NUMSEC 
Number of Sectors.  This field gives the ratio of the full circle to the
angular extension of the mesh.  This has to be a power of two.  For
example, NUMSEC = 4 means that the mesh of the part represents 
one fourth of the total circle.  If NUMSEC = 0 for *EM_2DAXI, the 
solver will replace it with this value.
*EM_SOLVER_BEM 
Purpose:  Define the type of linear solver and pre-conditioner as well as tolerance for the 
EM_BEM solve. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RELTOL  MAXITE 
STYPE 
PRECON  USELAS  NCYCLBEM 
Type 
I 
I 
Default 
1E-6 
1000 
I 
2 
I 
2 
I 
1 
I 
5000 
  VARIABLE   
RELTOL 
DESCRIPTION 
Relative tolerance for the iterative solvers (PCG or GMRES).  The
user  should  try  to  decrease  this  tolerance  if  the  results  are  not
accurate enough.  More iterations will then be needed. 
MAXITER 
Maximal number of iterations. 
STYPE 
Solver type: 
EQ.1: Direct  solve  –  the  matrices  will  then  be  considered  as 
dense. 
EQ.2: Pre-Conditioned Gradient method (PCG) - this allows to 
have block matrices with low rank blocks, and thus reduce
memory used. 
EQ.3: GMRES method - this allows to have block matrices with 
low  rank  blocks  and  thus  reduce  memory  used.    The
GMRES option only works in Serial for now. 
PRECON 
Preconditioner type for PCG or GMRES iterative solves: 
EQ.0: No preconditioner 
EQ.1: Diagonal line 
EQ.2: Diagonal block 
EQ.3: Broad diagonal including all neighbor faces 
EQ.4: LLT factorization.  The LLT factorization option only works
in serial for now.
VARIABLE   
DESCRIPTION 
USELAST 
This is used only for iterative solvers (PCG or GMRES). 
EQ.-1: Start  from  0  as  initial  guess  for  solution  of  the  linear 
system. 
EQ.1:  Starts from the previous solution normalized by the RHS
change. 
NCYLBEM 
Number  of  electromagnetism  cycles  between  the  recalculation  of
BEM matrices. 
Remarks: 
1.  Using USELAST = 1 can save many iterations in the subsequent solves if the vector 
solution of the present solve is assumed to be nearly parallel to the vector solution 
of the previous solve, as usually happens in time-domain eddy-current problems.  
2.  Since the BEM matrices depend on (and only on) the surface node coordinates of 
the conductors, it is important to recalculate them when the conductors are mov-
ing.    The  frequency  with  which  they are  updated  is  controlled  by  NCYLBEM.  
Note that very small values, for example NCYLBEM = 1, should, generally, be 
avoided since this calculation involves a high computational cost.  However, when 
two conductors are moving and in contact with each other it is recommended to 
recalculate the matrices at every time step.
*EM_SOLVER_BEMMAT 
Purpose:  Define the type of BEM matrices as well as the way they are assembled. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MATID 
Type 
I 
Default 
none 
RELTOL 
F 
1E-6 
  VARIABLE   
DESCRIPTION 
MATID 
Defines which BEM matrix the card refers to: 
EQ.1: 𝐏 matrix 
EQ.2: 𝐐 matrix 
RELTOL 
Relative tolerance on the sub-blocks of the matrix when doing low 
rank  approximations.    The  user  should  try  to  decrease  these
tolerances if the results are not accurate enough.  More memory will
then be needed.
*EM 
Purpose:  Define some parameters for the EM_FEM solver. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RELTOL  MAXITE 
STYPE 
PRECON  USELAST NCYCLFEM 
Type 
I 
I 
Default 
10-3 
1000 
I 
1 
I 
1 
I 
1 
I 
5000 
  VARIABLE   
RELTOL 
DESCRIPTION 
Relative tolerance for the iterative solvers (PCG or GMRES).  The
user  should  try  to  decrease  this  tolerance  if  the  results  are  not
accurate enough.  More iterations will then be needed. 
MAXITER 
Maximal number of iterations. 
STYPE 
Solver type: 
EQ.1: Direct solve  
EQ.2: Conditioned Gradient Method (PCG) 
PRECON 
Preconditioner type for PCG. 
EQ.0: No preconditioner 
EQ.1: Diagonal line 
USELAST 
This is used only for iterative solvers (PCG). 
EQ.-1:  starts from 0 as initial solution of the linear system. 
EQ.1:  starts  from  previous  solution  normalized  by  the  right-
hand-side change change. 
NCYCLFEM 
Number  of  electromagnetism  cycles  between  the  recalculation  of
FEM matrices.
*EM_SOLVER_FEM 
1.  Using USELAST = 1 can save many iterations in the subsequent solves if the vector 
solution of the present solve is assumed to be nearly parallel to the vector solution 
of the previous solve, as usually happens in time-domain eddy-current problems. 
2.  The default values are only valid when the PCG resolution method (STYPE = 2).  
For the default direct solve (STYPE = 1) those values are ignored. 
3.  When  the  conductor  parts  are  deforming  or  undergoing  changes  in  their  EM 
material properties (conductivity for example), it is important to change the de-
fault value of NCYLFEM to recalculate the FEM matrices more often.
*EM 
Purpose:  Define some parameters for the coupling between the EM_FEM and EM_BEM 
solvers. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RELTOL  MAXITE 
FORCON 
Type 
F 
I 
Default 
1E-2 
50 
I 
0 
  VARIABLE   
RELTOL 
DESCRIPTION 
Relative tolerance for the solver.  The user should try to decrease
this tolerance if the results are not accurate enough.  More iterations
will then be needed. 
MAXITER 
Maximal number of iterations. 
FORCON 
EQ.0: the code stops with an error if no convergence 
EQ.1: the  code  continues  to  the  next  time  step  even  if  the
RELTOL convergence criteria has not been reached..
*EM_SOLVER_FEMBEM 
Purpose:  Impose a voltage drop between two segment sets. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VDID 
VDTYPE 
SSID1 
SSID2 
VOLT 
Type 
I 
I 
I 
I 
F 
Default 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
VDID 
Voltage Drop ID 
VDTYPE 
Voltage Drop Type: 
EQ.1:  Voltage drop between the two corresponding nodes of the 
two segment sets SSID1 and SSID2. 
SSID1 
SSID2 
VOLT 
Segment Set ID 1 
Segment Set ID 2 
Value of the voltage drop
*ICFD 
The keyword *ICFD covers all the different options available in the incompressible fluid 
solver.  The keyword cards in this section are defined in alphabetical order: 
*ICFD_BOUNDARY_CONJ_HEAT 
*ICFD_BOUNDARY_FLUX_TEMP 
*ICFD_BOUNDARY_FREESLIP 
*ICFD_BOUNDARY_FSI 
*ICFD_BOUNDARY_FSWAVE 
*ICFD_BOUNDARY_GROUND 
*ICFD_BOUNDARY_NONSLIP 
*ICFD_BOUNDARY_PRESCRIBED_MOVEMESH 
*ICFD_BOUNDARY_PRESCRIBED_PRE 
*ICFD_BOUNDARY_PRESCRIBED_TEMP 
*ICFD_BOUNDARY_PRESCRIBED_TURBULENCE 
*ICFD_BOUNDARY_PRESCRIBED_VEL 
*ICFD_BOUNDARY_WINDKESSEL 
*ICFD_CONTROL_ADAPT 
*ICFD_CONTROL_ADAPT_SIZE 
*ICFD_CONTROL_CONJ 
*ICFD_CONTROL_DEM_COUPLING 
*ICFD_CONTROL_FSI 
*ICFD_CONTROL_GENERAL 
*ICFD_CONTROL_IMPOSED_MOVE 
*ICFD_CONTROL_LOAD 
*ICFD_CONTROL_MESH
*ICFD_CONTROL_MESH_MOV 
*ICFD_CONTROL_MONOLITHIC 
*ICFD_CONTROL_OUTPUT 
*ICFD_CONTROL_OUTPUT_SUBDOM 
*ICFD_CONTROL_PARTITION 
*ICFD_CONTROL_POROUS 
*ICFD_CONTROL_STEADY 
*ICFD_CONTROL_SURFMESH 
*ICFD_CONTROL_TAVERAGE 
*ICFD_CONTROL_TIME 
*ICFD_CONTROL_TRANSIENT 
*ICFD_CONTROL_TURB_SYNTHESIS 
*ICFD_CONTROL_TURBULENCE 
*ICFD_DATABASE_AVERAGE 
*ICFD_DATABASE_DRAG 
*ICFD_DATABASE_FLUX 
*ICFD_DATABASE_HTC 
*ICFD_DATABASE_NODEAVG 
*ICFD_DATABASE_NODOUT 
*ICFD_DATABASE_POINTAVG 
*ICFD_DATABASE_POINTOUT 
*ICFD_DATABASE_RESIDUALS 
*ICFD_DATABASE_TEMP 
*ICFD_DATABASE_TIMESTEP 
*ICFD_DATABASE_UINDEX 
*ICFD_DEFINE_NONINERTIAL
*ICFD_DEFINE_POINT 
*ICFD_DEFINE_WAVE_DAMPING 
*ICFD_INITIAL 
*ICFD_INITIAL_TURBULENCE 
*ICFD_MAT 
*ICFD_MODEL_NONNEWT 
*ICFD_MODEL_POROUS 
*ICFD_PART 
*ICFD_PART_VOL 
*ICFD_SECTION 
*ICFD_SET_NODE 
*ICFD_SOLVER_SPLIT 
*ICFD_SOLVER_TOL_MMOV 
*ICFD_SOLVER_TOL_MOM 
*ICFD_SOLVER_TOL_MONOLITHIC 
*ICFD_SOLVER_TOL_PRE 
*ICFD_SOLVER_TOL_TEMP
*ICFD_BOUNDARY_CONJ_HEAT 
Purpose:  Specify which boundary of the fluid domain will exchange heat with the solid. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
Type 
I 
Default 
none 
  VARIABLE   
DESCRIPTION 
PID 
PID of the fluid surface in contact with the solid.
*ICFD 
Purpose:  Impose a heat flux on the boundary expressed as 𝑞 = ∇𝑇 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
Variable 
PID 
LCID 
Type 
I 
I 
3 
SF 
F 
4 
5 
6 
7 
8 
DEATH 
BIRTH 
F 
F 
Default 
none 
none 
1. 
1.E+28
0.0 
  VARIABLE   
DESCRIPTION 
PID 
LCID 
PID for a fluid surface. 
*DEFINE_CURVE, 
Load curve ID to describe the temperature flux value versus time,
or
see 
*DEFINE_FUNCTION.  .    If  a  DEFINE_FUNCTION  is  used,  the 
following 
allowed:
 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑡𝑖𝑚𝑒).   
*DEFINE_CURVE_FUNCTION 
parameters 
are 
SF 
Load curve scale factor.  (default = 1.0) 
DEATH 
Time at which the imposed motion/constraint is removed: 
EQ.0.0:  default set to 10e28 
BIRTH 
Time at which the imposed pressure is activated starting from the 
initial abscissa value of the curve
*ICFD_BOUNDARY_FREESLIP  
Purpose:  Specify the fluid boundary with free-slip boundary condition. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
Type 
I 
Default 
none 
  VARIABLE   
PID 
DESCRIPTION 
PID  of  the  fluid  surface  where  a  free-slip  boundary  condition  is 
applied.
*ICFD 
Purpose:  This keyword defines which fluid surfaces will be considered in contact with the 
solid surfaces for fluid-structure interaction (FSI) analysis.  This keyword should not be 
defined if *ICFD_CONTROL_FSI is not defined. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
Type 
I 
Default 
none 
  VARIABLE   
DESCRIPTION 
PID 
PID of the fluid surface in contact with the solid domain.
*ICFD_BOUNDARY_FSWAVE 
Purpose:  Impose a wave inflow boundary condition.   
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
WTYPE 
HEIGHT 
WAMP 
WLENG 
WANG 
SFLCID 
Type 
I 
I 
F 
F 
F 
F 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
PID 
PID for a fluid surface. 
WTYPE 
Wave Type: 
EQ.1: Stokes wave of first order 
EQ.2: Stokes wave of second order 
HEIGHT 
Free surface equilibrium level 
WAMP 
Wave amplitude 
WLENG 
Wave Length 
WANG 
Wave Incidence Angle (3D only) 
SFLCID 
Scale factor LCID on the wave amplitude
*ICFD 
Purpose:  Specify the fluid boundary with a ground boundary condition.  The ground 
boundary condition is similar to the nonslip boundary condition except that it will keep 
V = 0 in all circumstances, even if the surface nodes are moving.  This is useful in cases 
where 
(using 
ICFD_BOUNDARY_PRESCRIBED_MOVEMESH for example) but those displacements are 
only to accommodate for mesh movement and do not correspond to a physical motion.   
to  move 
translate 
allowed 
nodes 
the 
are 
or 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
Type 
I 
Default 
none 
  VARIABLE   
PID 
DESCRIPTION 
PID  of  the  fluid  surface  where  a  ground  boundary  condition  is 
applied.
*ICFD_BOUNDARY_NONSLIP 
Purpose:  Specify the fluid boundary with a non-slip boundary condition. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
Type 
I 
Default 
none 
  VARIABLE   
PID 
DESCRIPTION 
PID  of  the  fluid  surface  where  a  non-slip  boundary  condition  is 
applied.
*ICFD_BOUNDARY_PRESCRIBED_MOVEMESH 
Purpose:  Allows the node of a fluid surface to translate in certain directions using an ALE 
approach.  This is useful in piston type applications or can also be used in certain cases to 
avoid big mesh deformation. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
dofx 
dofy 
dofz 
Type 
I 
Default 
none 
I 
1 
I 
1 
I 
1 
  VARIABLE   
DESCRIPTION
PID 
PID for a fluid surface. 
dofx, dofy, 
dofz 
Degrees of freedom in the X,Y and Z directions : 
EQ.0:  degree of freedom left free (Surface nodes can translate in
the chosen direction) 
EQ.1:  prescribed degree of freedom (Surface nodes are blocked)
*ICFD_BOUNDARY_PRESCRIBED_PRE 
Purpose:  Impose a fluid pressure on the boundary. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
Variable 
PID 
LCID 
Type 
I 
I 
3 
SF 
F 
4 
5 
6 
7 
8 
DEATH 
BIRTH 
F 
F 
Default 
none 
none 
1. 
1.E+28
0.0 
  VARIABLE   
DESCRIPTION 
PID 
LCID 
PID for a fluid surface. 
Load curve ID to describe the pressure value versus time, see *DE-
or
FINE_CURVE, 
*DEFINE_FUNCTION.    .  If  a  DEFINE_FUNCTION  is  used,  the
following 
allowed:
 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑡𝑖𝑚𝑒).   
*DEFINE_CURVE_FUNCTION 
parameters 
are 
SF 
Load curve scale factor.  (default = 1.0) 
DEATH 
Time at which the imposed motion/constraint is removed: 
EQ.0.0:  default set to 10E28 
BIRTH 
Time at which the imposed pressure is activated starting from the 
initial abscissa value of the curve
*ICFD_BOUNDARY_PRESCRIBED_TEMP 
Purpose:  Impose a fluid temperature on the boundary. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
Variable 
PID 
LCID 
Type 
I 
I 
3 
SF 
F 
4 
5 
6 
7 
8 
DEATH 
BIRTH 
F 
F 
Default 
none 
none 
1. 
1.E+28
0.0 
  VARIABLE   
DESCRIPTION 
PID 
LCID 
PID for a fluid surface. 
Load curve ID to describe the temperature value versus time; see
or
*DEFINE_CURVE, 
*DEFINE_FUNCTION.  .    If  a  DEFINE_FUNCTION  is  used,  the 
following 
allowed:
 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑡𝑖𝑚𝑒).   
*DEFINE_CURVE_FUNCTION 
parameters 
are 
SF 
Load curve scale factor.  (default = 1.0) 
DEATH 
Time at which the imposed temperature is removed: 
EQ.0.0:  default set to 10E28 
BIRTH 
Time at which the imposed temperature is activated starting from 
the initial abscissa value of the curve
*ICFD_BOUNDARY_PRESCRIBED_TURBULENCE 
Purpose:    Optional  keyword  that  allows  the  user  to  strongly  impose  the  turbulence 
quantities when a RANS turbulence model is selected.  See ICFD_CONTROL_TURBU-
LENCE.  Mainly used to modify the default boundary conditions at the inlet. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
VTYPE 
IMP 
LCID 
Type 
I 
I 
Default 
none 
none 
I 
0 
I 
none 
  VARIABLE   
DESCRIPTION 
PID 
PID for a fluid surface. 
VTYPE 
Variable type. 
EQ.1: kinetic turbulent energy 
EQ.2: turbulent dissipation rate 
EQ.3:  specific dissipation rate 
EQ.4: modified turbulent viscosity 
IMP 
Imposition method. 
EQ.0:  Direct imposition through value specified by LCID 
EQ.1: Using turbulent Intensity specified by LCID if VTYPE = 1. 
Using  turbulence  length  scale  specified  by  LCID  if
VTYPE = 2,3 and 4.  
EQ.2:  Using turbulent viscosity ratio specified by  LCID.  Only
available for VTYPE = 2 and VTYPE = 3. 
LCID 
Load curve ID to describe the variable value versus time, see *DE-
FINE_CURVE, *DEFINE_CURVE_FUNCTION or *DEFINE_FUNC-
TION.  . If a DEFINE_FUNCTION is used, the following parameters 
are allowed: 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑡𝑖𝑚𝑒, 𝑘, 𝑒, 𝑚𝑢𝑡).
Remarks: 
1.  At  the  inlet,  the  relationship  between  the  turbulent  kinetic  energy  𝑘  and  the 
turbulence intensity 𝐼 is given by : 
𝑘 =
(𝑈𝑎𝑣𝑔
2𝐼2) 
By default, the solver uses an inlet intensity of 0.05 (5%). 
2.  At the inlet, if specifying the turbulent dissipation rate using a length scale, 𝑙, the 
following relationship will be used : 
𝜖 = 𝐶𝜇
3/4 𝑘3/2
By default, the solver estimates a length scale based on the total height of the chan-
nel.  Otherwise, if using the turbulent viscosity ratio 𝑟 =
𝜇𝑡
𝜇  method: 
𝜖 = 𝜌𝐶𝜇
𝑘2
𝜇 𝑟
3.  At the inlet, if specifying the specific dissipation rate using a length scale, 𝑙, the 
following relationship will be used : 
𝜔 = 𝐶𝜇
−1/4 𝑘1/2
By default, the solver estimates a length scale based on the total height of the chan-
nel.  Otherwise, if using the turbulent viscosity ratio 𝑟 =
𝜇𝑡
𝜇  method: 
LS-DYNA R10.0 
5-15 (ICFD) 
𝜔 = 𝜌
4.  At the inlet, the relationship between the modified turbulent viscosity 𝜈̃ is given 
and the  length scale, 𝑙 is given by : 
𝜈̃ = 0.05√
(𝑈𝑎𝑣𝑔 𝑙)
*ICFD_BOUNDARY_PRESCRIBED_VEL 
Purpose:  Impose the fluid velocity on the boundary. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
Variable 
PID 
DOF 
VAD 
LCID 
Type 
I 
I 
Default 
none 
none 
I 
1 
I 
none 
1. 
5 
SF 
F 
6 
7 
8 
VID 
DEATH 
BIRTH 
I 
0 
F 
F 
1.E+28 
0.0 
  VARIABLE   
DESCRIPTION 
PID 
DOF 
PID for a fluid surface. 
Applicable degrees of freedom: 
EQ.1:  𝑥- degree of freedom, 
EQ.2:  𝑦- degree of freedom, 
EQ.3:  𝑧 degree of freedom, 
EQ.4:  Normal direction degree of freedom, 
VAD 
Velocity flag: 
EQ.1: Linear velocity 
EQ.2: Angular velocity 
EQ.3: Parabolic velocity profile 
EQ.4: Activates  synthetic  turbulent  field  on  part.    See  *ICFD_-
CONTROL_TURB_SYNTHESIS. 
Load curve ID used to describe motion value versus time, see *DE-
FINE_CURVE, *DEFINE_CURVE_FUNCTION, or *DEFINE_FUNC-
TION.  If a DEFINE_FUNCTION is used, the following parameters 
are allowed:  𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑡𝑖𝑚𝑒).   
Load curve scale factor.  (default = 1.0) 
Point  ID  for  angular  velocity  application  point,  see  *ICFD_DE-
FINE_POINT. 
LCID 
SF 
VID
*ICFD_BOUNDARY_PRESCRIBED_VEL 
DESCRIPTION 
DEATH 
Time at which the imposed motion/constraint is removed: 
EQ.0.0:  default set to 1028 
BIRTH 
Time at which the imposed motion/constraint is activated starting 
from the initial abscissa value of the curve
*ICFD 
Purpose:  This boundary condition imposes the pressure function of circuit parameters 
where an analogy is made between the pressure and scalar potential as well as between the 
flux and the current intensity.  Such conditions are frequently encountered in hemodynam-
ics.  
  Card 1 
1 
2 
Variable 
PID 
WTYPE 
Type 
I 
I 
3 
R1 
F 
Default 
none 
none 
0. 
4 
C1 
F 
0. 
5 
R2 
F 
0. 
6 
L1 
F 
0. 
7 
8 
4 
5 
6 
7 
8 
Optional card if WTYPE = 3 or 4. 
  Card 2 
1 
Variable 
P2LCID 
Type 
I 
2 
C2 
F 
Default 
None 
0. 
3 
R3 
F 
0. 
  VARIABLE   
DESCRIPTION 
PID 
PID for a fluid surface 
WTYPE 
Circuit type  : 
EQ.1:  Windkessel circuit 
EQ.2:  Windkessel circuit with inverted flux 
EQ.3:  CV type circuit 
EQ.4:  CV type circuit with inverted flux 
R1/C1/L1/R
2/C2 
Parameters (Resistances, inductances, capacities) for the different
circuits. 
P2LCID 
Load curve ID describing behavior of P2(t) function of time for CV
type circuit.
i(t)
R2
P(t)
Meshed 
Part
C1
R1
L1
Figure 5-1. Windkessel Circuit 
Remarks: 
1.  Figure 5-1 shows a Windkessel circuit and Figure 5-2 a CV circuit. 
i(t)
R1
R2
P(t)
Meshed 
Part
C1
C2
R3
P2(t)
Figure 5-2.  CV Circuit
*ICFD 
Purpose:  This keyword will activate the adaptive mesh refinement feature.  The solver will 
use an a-posteriori error estimator to compute a new mesh size bounded by the user to 
satisfy a maximum perceptual global error. 
  Card 1 
1 
2 
3 
4 
Variable 
MINH 
MAXH 
ERR 
MTH 
Type 
F 
F 
F 
Default 
none 
none 
none 
I 
0 
5 
NIT 
I 
0 
6 
7 
8 
  VARIABLE   
MINH 
DESCRIPTION 
Minimum mesh size allowed to the mesh generator.  The resulting
mesh  will  not  have  an  element  smaller  than  MINH  even  if  the
minimum size does not satisfy the maximum error. 
MAXH 
Maximum mesh size. 
ERR 
MTH 
Maximum perceptual error allowed in the whole domain. 
Specify  if  the  mesh  size  is  computed  based  on  function  error  or
gradient error. 
EQ.0: Function error. 
EQ.1: Gradient error. 
NIT 
Number of iterations before a re-meshing is forced.  Default forces a 
re-meshing at every timestep.
*ICFD_CONTROL_ADAPT_SIZE 
Purpose:    This  keyword  controls  the  re-meshing  of  elements  taking  into  account  the 
element quality and distortion in contrast to the default algorithm which only checks for 
inverted elements. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ASIZE 
NIT 
Type 
Default 
I 
0 
I 
none 
  VARIABLE   
ASIZE 
DESCRIPTION 
EQ.0: only re-mesh in cases where elements invert. 
EQ.1: re-mesh  if  elements  invert  or  if  element  quality  deterio-
rates. 
NIT 
Number of iterations before a re-meshing is forced.  If a negative 
integer is entered, then a load curve function of time will be used to
define NIT.
*ICFD 
Purpose:    This  keyword  allows  to  pick  between  the  different  coupling  methods  for 
conjugate heat transfer applications 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
CTYPE 
Type 
Default 
I 
0 
  VARIABLE   
DESCRIPTION 
CTYPE 
Indicates the thermal coupling type. 
EQ.0: Robust  and  accurate  monolithic  coupling  where  the
temperature field are solved simultaneously between the
fluid and the structure.  
EQ.1: Weak thermal coupling.  The fluid passes the heat flux to
the solid at the fluid-structure interface and the solid re-
turns the temperature which is applied as a Dirichlet condi-
tion. 
Remarks: 
1.  The keyword ICFD_BOUNDARY_CONJ_HEAT is ignored if CTYPE = 1 but the 
keyword ICFD_BOUNDARY_FSI is needed in all thermal coupling cases.
*ICFD_CONTROL_DEM_COUPLING 
Purpose:  This keyword is needed to activate coupling between the ICFD and DEM solvers. 
5 
6 
7 
8 
  Card 1 
1 
Variable 
CTYPE 
Type 
Default 
I 
0 
2 
BT 
F 
3 
DT 
F 
4 
SF 
F 
0. 
1E+28 
1. 
  VARIABLE   
DESCRIPTION 
CTYPE 
Indicates the coupling direction to the solver. 
EQ.0:  two-way  coupling  between  the  fluid  and  the  solid 
particles. 
EQ.1:  one-way coupling: 
The DEM particles transfer their 
location to the fluid solver. 
EQ.2: one-way coupling: 
the DEM particles 
The fluid solver transfers forces to 
BT 
DT 
SF 
Birth time for the DEM coupling.  
Death time for the DEM coupling.  
Scale  force  which  can  be  applied  on  the  force  by  to  the  DEM
particles.
*ICFD 
Purpose:  This keyword modifies default values for the fluid-structure interaction coupling 
algorithm. 
4 
5 
6 
7 
8 
IDC 
LDICSF 
XPROJ 
  Card 1 
1 
Variable 
OWC 
Type 
Default 
I 
0 
2 
BT 
F 
0 
3 
DT 
F 
F 
I 
0 
I 
0 
1E+28 
0.25 
  VARIABLE   
DESCRIPTION 
OWC 
Indicates the coupling direction to the solver. 
EQ.0: two-way coupling: 
Loads  and  displacements  are 
transferred across the FSI interface and the full non-linear 
problem is solved. 
EQ.1: one-way coupling: 
The  solid  mechanics  solver 
transfers displacements to the fluid solver. 
EQ.2: one-way coupling: 
The fluid solver transfers stresses 
to the solid mechanics solver. 
BT 
DT 
Birth time for the FSI coupling.  Before BT the fluid solver will not
pass  any  loads  to  the  structure  but  it  will  receive  displacements
from the solid mechanics solver. 
Death time for the FSI coupling.  After DT the fluid solver will not
transfer any loads to the solid mechanics solver but the fluid will
continue to deform with the solid. 
IDC 
Interaction detection coefficient.  See Remark 1. 
LCIDSF 
Optional  load  curve  ID  to  apply  a  scaling  factor  on  the  forces
transferred to the solid : 
GT.0: Load curve ID function of iterations 
LT.0:  Load curve ID function of time
Fluid Nodes
Solid Nodes
Figure 5-3.  Geometry of FSI contact. 
DESCRIPTION 
Projection  of  the  nodes  of  the  CFD  domain  that  are  at  the  FSI 
interface onto the structural mesh. 
EQ.0: No projection  
EQ.1: Projection 
  VARIABLE   
XPROJ 
Remarks: 
1.  One of the criteria to automatically detect the fluid and solid surfaces that will 
interact in FSI problems is the distance 𝑑 between a fluid (solid) node and a solid 
(fluid) element respectively: 
𝑑 ≤ IDC × min (ℎ, 𝐻) 
where ℎ is the size of the fluid mesh, 𝐻 the size of the solid mechanics mesh, and 
IDC a detection coefficient criteria with IDC = 0.25 by default.  In the majority of 
cases, this default value is sufficient to ensure FSI interaction.  However, it can 
happen in special cases that the fluid and solid geometries have curvatures that 
differ too much (example: pipe flows in conjugate heat transfer applications).  In 
such cases, a bigger IDC value may be needed.  This flag should be handled with 
care. 
2.  XPROJ = 1 is recommended for cases with rotation.
*ICFD 
Purpose:    This  keyword  allows  choosing  between  the  different  types  of  CFD  analyses 
(transient or steady state). 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ATYPE 
MTYPE 
Type 
Default 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION 
ATYPE 
Analysis type : 
EQ.  -1: Turns off the ICFD solver after initial keyword reading.
EQ.0: Transient analysis (Default) 
MTYPE 
Solving Method type : 
EQ.0: Fractional Step Method 
EQ.1: Monolithic solve 
    EQ.2: Potential flow solve (Steady state only)
*ICFD_CONTROL_IMPOSED_MOVE 
Purpose:  This keyword allows the user to impose a velocity on specific ICFD parts or on 
the whole volume mesh.  Global translation, global rotation and local rotation components 
can be defined and combined.  This can be used in order to save calculation time in certain 
applications such as sloshing where the modeling of the whole fluid box and the solving of 
the consequent FSI problem is not necessarily needed. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
LCVX 
LCVY 
LCVZ 
VADT 
Type 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
I 
0 
Optional Card. Rotational velocity components using Euler angles . 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ALPHAL 
BETAL 
GAMMAL
ALPHAG 
BETAG  GAMMAG 
VADR 
Type 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
I 
0 
Optional Card. Local reference frame definition if ALPHAL, BETAL or GAMMAL used.
  Card 3 
1 
Variable 
PTID 
Type 
Default 
I 
0 
2 
X1 
F 
1. 
3 
Y1 
F 
0. 
4 
Z1 
F 
0. 
5 
X2 
F 
0. 
6 
Y2 
F 
1. 
7 
Z2 
F 
0.
VARIABLE   
PID 
DESCRIPTION 
PID.    This  can  be  any  part  ID  referenced  in
*ICFD_PART or *ICFD_PART_VOL.  If PID = 0, 
then the whole volume mesh will be used. 
LCVX, LCVY, LCVZ 
LCID for the velocity in the three global directions
(𝑥, 𝑦, 𝑧). 
VADT 
Velocity/Displacements 
components 
flag 
for 
translation 
EQ.0: Prescribe Velocity  
EQ.1: Prescribe Displacements 
ALPHAL, BETAL, GAMMAL 
LCID for the three Euler angle rotational velocities
in the local reference frame . 
ALPHAG, BETAG, GAMMAG 
LCID for the three Euler angle rotational velocities
in the global reference frame . 
VADR 
Velocity/Displacements 
components 
flag 
for 
rotation
EQ.0: Prescribe Velocity  
EQ.1: Prescribe Displacements 
Point ID for the origin of the local reference frame. 
If not defined, the barycenter of the volume mesh
will be used. 
Three components of the local reference X1 axis.
If not defined, the global 𝑥 axis will be used. 
Three components of the local reference X2 axis.
If not defined, the global 𝑦 axis will be used. 
PTID 
X1, Y1, Z1 
X2, Y2, Z2 
Remarks:
Figure 5-4.  A rotation represented by Euler angles (𝛼, 𝛽, 𝛾) using 𝐙(𝛼)𝐗(𝛽)𝐙(𝛾)
intrinsic rotations. 
1.  Rotations.  Any target orientation can be reached starting from a known reference 
orientation using a specific sequence of intrinsic rotations whose magnitudes are 
the Euler angles (𝛼, 𝛽, 𝛾).  Equivalently, any rotation matrix R can be decomposed 
as a product of three elemental rotation matrices.  For instance: 
𝐑 = 𝐗(𝛼)𝐘(𝛽)𝐙(𝛾) 
However, different definition of the elemental rotation matrices (𝑥, 𝑦, 𝑧) and their 
multiplication order can be adopted.  The ICFD solver uses the following approach 
and rotation matrix: 
𝐙(𝛼)𝐗(𝛽)𝐙(𝛾) =
⎡
⎢
⎢
⎢
⎢
⎣
𝑐𝛼𝑐γ − 𝑐𝛽𝑠𝛼𝑠𝛾 −𝑐𝛽𝑐𝛾𝑠𝛼 − 𝑐𝛼𝑠𝛾
𝑐γ𝑠𝛼 + 𝑐𝛼𝑐𝛽𝑠𝛾
𝑐𝛼𝑐𝛽𝑐𝛾 − 𝑠𝛼𝑠𝛾 −𝑐𝛼𝑠𝛽
𝑠𝛽𝑠𝛾
𝑐𝛾𝑠𝛽
𝑠𝛼𝑠𝛽
⎤
⎥
⎥
⎥
⎥
𝑐𝛽 ⎦
where 𝑿(𝛼), 𝒀 (𝛽), and 𝒁(𝛾) are the matrices representing the elemental rotations 
about the axes (𝑥, 𝑦, 𝑧), 𝑠𝛼 = sin(𝛼), and 𝑐𝛽 = cos(𝛽). 
2.  Local  Coordinate  Systems.    It  is  possible  to  have  the  ICFD  parts  or  ICFD_-
PART_VOLs rotate around the global reference frame but also to define and use a 
local  reference  frame  by  defining  its  point  of  origin  and  two  of  its  vectors 
𝐯1 = (X1, Y1, Z1) and 𝐯2 = (X2, Y2, Z2).  The third vector is, then, in the direction 
of 𝐯1 × 𝐯2.  See Figure 5-4.
*ICFD 
Purpose:  This keyword resets the body load in the ICFD solver to zero, while leaving the 
body load unchanged for the solid mechanics solver.  It is useful in problems where the 
gravity acceleration may be neglected for the fluid problem, but not for the solid mechanics 
problem. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ABL 
Type 
Default 
I 
1 
  VARIABLE   
ABL 
DESCRIPTION 
EQ.0: the body load provided in *LOAD_BODY is reset to zero 
only for the fluid analysis.
*ICFD_CONTROL_MESH 
Purpose:  This keyword modifies default values for the automatic volume mesh generation.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MGSF 
MSTRAT  2DSTRUC NRMSH 
Type 
F 
Default 
1.41 
I 
0 
I 
0 
I 
0 
  VARIABLE   
MGSF 
DESCRIPTION 
Mesh Growth Scale Factor : Specifies the maximum mesh size that
the volume mesher is allowed to use when generating the volume
mesh based on the mesh surface element sizes defined in *MESH_-
SURFACE_ELEMENT. 
MSTRAT 
Mesh generation strategy : 
EQ.0: Mesh generation based on Delaunay criteria  
EQ.1: Mesh generation based on octree  
2DSTRUC 
Flag to decide between a unstructured mesh generation strategy in
2D or a structured mesh strategy : 
EQ.0: Structured mesh  
EQ.1: Unstructured mesh 
NRMSH 
Flag to turn off any remeshing : 
EQ.0: Remeshing possible 
EQ.1: Remeshing impossible 
Remarks: 
1.  For MGSF, values between 1 and 2 are allowed.  Values closer to 1 will result in a 
finer volume mesh (1 means the volume mesh is not allowed to be coarser than the 
element size from the closest surface meshes) and values closer to 2 will result in a 
coarser volume mesh (2 means the volume can use elements as much as twice as 
coarse as those from the closest surface mesh).  MGSF has a fixed value of 1 in 2D.
2. 
If the user knows in advance that no remeshing will occur during the analysis, 
then setting NRMSH to 1may be useful as it will free space used to back up the 
mesh and consequently lower memory consumption. 
3.  The Default Mesh generation strategy (based on Delaunay criteria) yields a linear 
interpolation of the mesh size between two surfaces facing each other whereas the 
octree based generation strategy allows for elements’ sizes to remain close to the 
element surface mesh size over a longer distance.  This can be useful in configura-
tions where two surface meshes facing each other have very distinct sizes in order 
to create a smoother transition.
*ICFD_CONTROL_MESH_MOV 
Purpose:  With this keyword the user can choose the type of algorithm for mesh movement. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MMSH 
LIM_ITER  RELTOL 
Type 
Default 
I 
2 
I 
F 
100 
1.0e-3 
VARIABLE 
MMSH 
DESCRIPTION 
Mesh motion selector: 
EQ.-1: Completely shuts off any mesh movement.   
EQ.1:  mesh moves based on the distance to moving walls. 
EQ.2:  mesh moves by solving a linear elasticity problem using
the element sizes as stiffness.(default) 
EQ.3:  mesh uses a Laplacian smoothing with stiffness on edges 
and from node to opposite faces.  Very robust, but costly.
EQ.4:  full Lagrangian:  The mesh moves with the velocity of the 
flow. 
EQ.11:  mesh moves using an implicit ball-vertex spring method.
LIM_ITER 
RELTOL 
Maximum  number  of  linear  solver  iterations  for  the  ball-vertex 
linear system. 
Relative tolerance to use as a stopping criterion for the ball-vertex 
method  iterative  linear  solver  (conjugate  gradient  solver  with
diagonal scaling preconditioner).
*ICFD 
Purpose:    This  keyword  allows  to  choose  between  the  Fractional  Step  Solver  and  the 
Monolithic Solver. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
Type 
Default 
I 
0 
  VARIABLE   
DESCRIPTION 
SID 
Solver ID : 
EQ.0: Fractional Step Solver.  Default. 
EQ.1: Monolithic Solver.
*ICFD_CONTROL_OUTPUT 
Purpose:  This keyword modifies default values for screen and file outputs related to this 
fluid solver only. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MSGL 
OUTL 
DTOUT 
LSPPOUT
ITOUT 
Type 
Default 
I 
0 
I 
0 
F 
0 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION 
MSGL 
Message level. 
EQ.0: only time step information is output. 
EQ.1: first level solver information. 
EQ.2: full output information with details about linear algebra
and convergence steps. 
EQ.4: full output information is also copied to the messag file.
OUTL 
Output the fluid results in other file formats apart from d3plot. 
EQ.0: only d3plot output 
EQ.2: output a file with mesh statistics and the fluid results in
OpenDX format.  A directory named dx will be created in 
the work directory where the output files will be written.
EQ.6: output a file with mesh statistics and the fluid results in
VTK format readable by Paraview.  A directory named vtk
will be created in the work directory where the output files
will be written. 
EQ.7:  output  a  file  with  mesh  statistic  and  the  fluid  results  in 
VTU format readable by Paraview.  A directory named vtk
will be created in the work directory where the output files
will be written. 
DTOUT 
Time interval to print the output when OUTL is different than 0.
VARIABLE   
LSPPOUT 
ITOUT 
.
DESCRIPTION 
EQ.1: outputs a file with the automatically created fluid volume
mesh in  a format compatible for LSPP. 
Iteration interval to print the output, including the d3plot files when
the 
. 
selected 
steady 
state 
is
*ICFD_CONTROL_OUTPUT_SUBDOM 
Purpose:    Defines  a  specific  zone  that  should  be  output  in  the  format  specified  by  the 
ICFD_CONTROL_OUTPUT card rather than the whole domain.  
Remeshing Control. First card specifies the shape of the output sub domain. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SNAME 
Type 
A 
Default 
none 
Box Case. Card 2 for Sname = box 
  Cards 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PMINX 
PMINY 
PMINZ 
PMAXX 
PMAXY 
PMAXZ 
Type 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
Sphere Case. Card 2 for Sname = sphere 
  Cards 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RADIUS  CENTERX  CENTERY  CENTERZ
Type 
F 
F 
F 
F 
Default 
none 
none 
none 
none
Cylinder Case. Card 2 for Sname = cylinder 
  Cards 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Radius 
PMINX 
PMINY 
PMAXZ 
PMAXX 
PMAXY 
PMAXZ 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
SNAME 
Shape name.  Possibilities include ‘box’, ‘cylinder’ and ‘sphere’
PMINX, Y, Z] 
X, Y, Z for the point of minimum coordinates 
PMAX[X, Y, Z] 
X, Y, Z for the point of maximum coordinates 
CENTER[X, Y, Z] 
Coordinates of the sphere center in cases where Sname is Sphere
RADIUS 
Radius of the sphere if SNAME  is sphere or of the cross section 
disk if SNAME is cylinder.
*ICFD_CONTROL_PARTITION 
Purpose:  This keyword changes the default option for the partition in MPP, thus it is only 
valid in MPP. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PTECH 
Type 
Default 
I 
1 
  VARIABLE   
DESCRIPTION 
PTECH 
Indicates the type of partition. 
EQ.1: the library Metis is used. 
EQ.2: partition along the axis with higher aspect ratio. 
EQ.3: partition along X axis. 
EQ.4: partition along Y axis. 
EQ.5: partition along Z axis.
Purpose:  This keyword modifies the porous media solve.  
*ICFD 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable  PMSTYPE 
Type 
Default 
I 
0 
  VARIABLE   
DESCRIPTION 
PMSTYPE 
Indicates the porous media solve type. 
EQ.0: Anisotropic Generalized Navier-Stokes model for porous 
media    using  Fractional 
step method. 
EQ.1: Anisotropic Darcy-Forcheimer model using a Monolithic 
approach for the solve.  This method is better suited for 
very low Reynolds flows through porous media (Frequent-
ly encountered in Resin Transfer Molding (RTM) applica-
tions). 
Remarks: 
1.  When using the Anisotropic Darcy-Forcheimer model, the convective term in the 
Navier Stokes formulation is neglected.
*ICFD_CONTROL_STEADY 
Purpose:  This keyword allows to specify convergence options for the steady state solver. 
  Card 1 
Variable 
1 
ITS 
2 
3 
4 
5 
6 
7 
8 
TOL1 
TOL2 
TOL3 
REL1 
REL2 
UREL 
ORDER 
Type 
I 
F 
F 
F 
F 
F 
Default 
1e6 
1.e-3 
1.e-3 
1.e-3 
0.3 
0.7 
F 
1. 
I 
0 
  VARIABLE   
    ITS 
TOL1/2/3 
REL1/2 
UREL 
DESCRIPTION 
Maximum number of iterations to reach convergence. 
Tolerance  limits  for  the  momentum  pressure  and  temperature
equations respectfully. 
Relaxation  parameters  for  the velocity  and  pressure  respectfully.
Decreasing those values may add stability but more iterations may
be needed to reach convergence. 
Under relaxation parameter.  Lowering this value may improve the
final accuracy of the solution but more iterations may be needed to
achieve convergence. 
ORDER 
Analysis order : 
EQ.0:  Second order.  More accurate but more time consuming.
EQ.1:  First  order:  More  stable  and  faster  but  may  be  less
accurate.
*ICFD 
Purpose:  This keyword enables automatic surface re-meshing.  The objective of the re-
meshing is to improve the mesh quality on the boundaries.  It should not be used on a 
regular basis. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RSRF 
SADAPT 
Type 
Default 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION 
RSRF 
Indicates whether or not to perform a surface re-meshing. 
EQ.0: no re-meshing is applied. 
EQ.1: Laplacian smoothing surface remeshing 
EQ.2: Curvature preserving surface remeshing 
SADAPT 
Indicates whether or not to trigger adaptive surface remeshing. 
EQ.0:  no adaptive surface re-meshing is applied. 
EQ.1:  automatic surface remeshing when quality deteriorates (3D
only). 
.
*ICFD_CONTROL_TAVERAGE 
Purpose:  This keyword controls the restarting time for computing the time average values.  
By default, there is no restarting and the average quantities are given starting from 𝑡 = 0.  
This keyword can be useful in turbulent problems that admit a steady state. 
2 
3 
4 
5 
6 
7 
8 
  Card 1 
Variable 
1 
DT 
Type 
F 
Default 
none 
  VARIABLE   
DESCRIPTION 
DT 
Over each DT time interval, the average quantities are reset.
*ICFD 
Purpose:  This keyword is used to change the defaults related to time parameters in the 
fluid problem. 
  Card 1 
1 
Variable 
TTM 
Type 
F 
Default 
1028 
2 
DT 
F 
0 
3 
4 
5 
6 
7 
8 
CFL 
LCIDSF 
DTMIN 
DTMAX 
DTINIT 
TDEATH 
F 
1 
I 
F 
F 
F 
F 
none 
none 
none 
None 
1E28 
  VARIABLE   
DESCRIPTION 
TTM 
DT 
CFL 
LCIDSF 
DTMIN 
DTMAX 
DTINIT 
TDEATH 
Total time of simulation for the fluid problem. 
Time step for the fluid problem.  If different from zero, the time step
will be set constant and equal to this value.  If DT = 0, then the time 
step is automatically computed based on the CFL condition. 
CFL number for DT = 0.  In general, CFL specifies a scale factor that 
is applied to the time step.  When DT = 0, the time step is set to the 
maximum  value  satisfying  the  CFL  condition,  in  which  case  this
scale factor is equal to the CFL number. 
Load  Curve  ID  specifying  the  CFL  number  when  DT =  0  as  a 
function of time, and more generally LCIDSF specifies the time step
scale factor as the function of time. 
Minimum  time  step.    When  an  automatic  time  step  is  used  and
DTMIN is defined, the time step cannot drop below DTMIN. 
Maximum  time  step.    When  an  automatic  time  step  is  used  and
DTMAX is defined, the time step cannot increase beyond DTMAX.
Initial  time  step.    If  not  defined,  the  solver  will  automatically
determine  an  initial  timestep  based  on  the  flow  velocity  or
dimensions of the problem in cases where there is no inflow. 
Death time for the Navier Stokes solve.  After TDEATH, the velocity
and pressure will no longer be updated.  But the temperature and
other similar quantities still can.
*ICFD_CONTROL_TRANSIENT 
Purpose:    This  keyword  allows  to  specify  different  integration  scheme  options  for  the 
transient solver. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TORD 
FSORD 
Type 
Default 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION 
TORD 
Time integration order : 
EQ.0:  Second order. 
EQ.1:  First order. 
FSORD 
Fractional step integration order : 
EQ.0:  Second order. 
EQ.1:  First order.
*ICFD 
Purpose:  This keyword enables the user to modify the default values for the turbulence 
model.  
  Card 1 
1 
2 
3 
Variable 
TMOD 
SUBMOD  WLAW 
Type 
Default 
I 
0 
I 
1 
Optional card if TMOD = 1. 
  Card 2 
1 
2 
Variable 
Ce1 
Ce2 
Type 
F 
F 
I 
1 
3 
𝜎𝑒
F 
4 
KS 
F 
0. 
4 
𝜎𝑘
F 
5 
CS 
F 
0. 
5 
𝐶𝜇
F 
6 
7 
8 
LCIDS1 
LCID2 
I 
I 
none 
none 
6 
7 
8 
𝐶𝑐𝑢𝑡
F 
Default 
1.44 
1.92 
1.3 
1.0 
0.09 
-1. 
Optional card TMOD = 2 or TMOD = 3. 
2 
3 
4 
5 
6 
7 
8 
  Card 2 
Variable 
1 
Cs 
Type 
F 
Default 
0.18
Card 2 
Variable 
Type 
1 
𝛾 
F 
2 
𝛽01
F 
Default 
1.44 
0.072 
Optional card if TMOD = 4. 
  Card 3 
Variable 
1 
𝑎1 
Type 
F 
2 
𝛽02
F 
Default 
0.31 
0.0828 
Optional card if TMOD = 5. 
  Card 2 
1 
Variable 
𝐶𝑏1
2 
𝐶𝑏1
Type 
F 
F 
3 
𝜎𝜔1
F 
2 
3 
𝜎𝜔2
F 
2 
3 
𝜎𝜈
F 
*ICFD_CONTROL_TURBULENCE 
7 
8 
5 
∗ 
𝛽0
F 
6 
𝐶𝑐𝑢𝑡
F 
0.09 
-1. 
6 
7 
8 
5 
𝐶𝑙
F 
0.875 
5 
6 
7 
8 
𝐶𝑤1
𝐶𝑤2
4 
𝜎𝑘1
F 
2 
4 
𝜎𝑘2
F 
2 
4 
𝐶𝑣1
F 
F 
F 
Default 
0.1355 
0.622 
0.66 
7.2 
0.3 
2.0
VARIABLE   
DESCRIPTION 
TMOD 
Indicates what turbulence model will be used. 
EQ.0: Turbulence  model  based  on  a  variational  multiscale
approach is used by default. 
EQ.1: RANS 𝑘 - 𝜀 approach. 
EQ.2: LES Smagorinsky sub-grid scale model. 
EQ.3: LES Wall adapting local eddy-viscosity (WALE) model.
EQ.4:  RANS 𝑘 - 𝑤 approach. 
EQ.5:  RANS Spalart Allmaras approach. 
SUBMOD 
Turbulence sub-model.  If TMOD = 1 : 
EQ.1: 
EQ.2: 
Standard model 
Realizable model 
If TMOD = 4 : 
EQ.1: 
EQ.2: 
EQ.3: 
Standard Wilcox 98 model 
Standard Wilcox 06 model 
SST Menter 2003 
WLAW 
Law of the wall ID is RANS turbulence model selected : 
EQ.1: Standard classic law of the wall. 
EQ.2: Standard Launder and Spalding law of the wall. 
EQ.4: Non equilibrium Launder and Spalding law of the wall.
EQ.5: Automatic classic law of the wall. 
Roughness physical height and Roughness constant.  Only used if
RANS turbulence model selected. 
Load curve describing user defined source term in turbulent kinetic
energy  equation  function  of  time.    See  *DEFINE_CURVE,  *DE-
FINE_CURVE_FUNCTION,  or  *DEFINE_FUNCTION.    If  a  DE-
FINE_FUNCTION is used, the following parameters are allowed:
 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑡𝑖𝑚𝑒, 𝑘, 𝑒, 𝑚𝑢𝑡). 
KS/CS 
LCIDS1
LCIDS2 
*ICFD_CONTROL_TURBULENCE 
DESCRIPTION 
Load  curve  describing  user  defined  source  term  in  turbulent 
dissipation equation function of time.  See *DEFINE_CURVE, *DE-
FINE_CURVE_FUNCTION,  or  *DEFINE_FUNCTION.    If  a  DE-
FINE_FUNCTION is used, the following parameters are allowed:
 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑡𝑖𝑚𝑒, 𝑘, 𝑒, 𝑚𝑢𝑡). 
Ce1, Ce2, 𝜎𝑒, 
𝜎𝑘, 𝐶𝜇, 𝐶𝑐𝑢𝑡 
𝑘 - 𝜀 model constants 
Cs 
Smagorinsky constant if TMOD = 2 or WALE constant if TMOD = 3
𝑘 -𝜔 model constants 
Spalart-Allmaras constants 
𝛾, 𝛽01, 𝜎𝜔1, 
𝜎𝑘1, 𝛽0
∗, 𝑎1, 
𝛽02, 𝜎𝜔2, 𝜎𝑘2, 𝐶𝑙, 𝐶𝑐𝑢𝑡
𝐶𝑏1,𝐶𝑏2,𝜎𝜈,
𝐶𝑣1, 𝐶𝑤1𝐶𝑤2 
Remarks: 
1.  For  the  Standard  𝑘 - 𝜀  model,  the  following  two  equations  are  solved  for  the 
turbulent kinetic energy and the turbulent dissipation respectively 𝑘 and 𝜀  : 
𝜕𝑘
𝜕𝑡
+
𝜕(𝑘𝑢𝑖)
𝜕𝑥𝑖
=
𝜕
𝜕𝑥𝑗
[(
+
𝜇𝑡
𝜌 𝜎𝑘
)
𝜕𝑘
𝜕𝑥𝑗
] + 𝑃𝑘 + 𝑃𝑏 − 𝜖 + 𝑆𝑘 
𝜕𝜖
𝜕𝑡
+
𝜕(𝜖𝑢𝑖)
𝜕𝑥𝑖
=
𝜕
𝜕𝑥𝑗
[(
+
𝜇𝑡
𝜌 𝜎𝜖
)
𝜕𝜖
𝜕𝑥𝑗
] + 𝐶1𝜖
𝑃𝑘 − 𝐶2𝜀
𝜖2
+ 𝑆𝑒 
With 𝑃𝑘 the 𝑘 production term, 𝑃𝑏 the production term due to buoyancy and 𝑆𝑘, 𝑆𝑒 
are the user defined source terms. 𝑃𝑘 and 𝑃𝑏 are expressed as : 
𝑃𝑘 =
𝜇𝑡
𝑆2 
𝑃𝑏 =
𝛽𝜇𝑡
𝜌𝑃𝑟𝑡
𝑔𝑖
𝜕𝑇
𝜕𝑥𝑖
With 𝑆 the modulus of the mean rate of strain tensor (𝑆2 = 2𝑆𝑖𝑗𝑆𝑖𝑗), 𝛽 the coefficient 
of thermal expansion, and 𝑃𝑟𝑡 the turbulent Prandtl number.  The turbulent viscosi-
ty is then expressed as:
𝜇𝑡 = 𝜌𝐶𝜇
𝑘2
For the realizable 𝑘 - 𝜀 model, the equation for the turbulent kinetic energy does not 
change, but the equation for the turbulent dissipation is now expressed as: 
𝜕𝜖
𝜕𝑡
+
𝜕(𝜖𝑢𝑖)
𝜕𝑥𝑖
=
𝜕
𝜕𝑥𝑗
[(
+
𝜇𝑡
𝜌 𝜎𝜖
)
𝜕𝜖
𝜕𝑥𝑗
] + 𝐶1𝑆𝜖 − 𝐶2𝜀
𝜖2
𝑘 + √
𝜌 𝜖
− 𝜖 + 𝑆𝑒 
With 𝐶1 = 𝑚𝑎𝑥[0.43,
𝜂+5],  𝜂 = 𝑆 𝑘
𝜖. 
Furthermore, while the turbulent viscosity is still expressed the same way, 𝐶𝜇 is no longer a 
constant: 
𝐶𝜇 =
𝐴0 + 𝐴𝑠𝑘 𝑈∗
𝑈∗ = √Ω𝑖𝑗Ω𝑖𝑗 + 𝑆𝑖𝑗𝑆𝑖𝑗 
𝐴0 = 4.04 
𝐴𝑠 = √6𝑐𝑜𝑠 (1
3 𝑐𝑜𝑠−1 (√6
𝑆𝑖𝑗𝑆𝑗𝑘𝑆𝑘𝑖
(𝑆𝑖𝑗𝑆𝑖𝑗)3/2)) 
It can be noted that in this case, the constant value 𝐶𝜇 that can be input by the user serves 
as the limit values that 𝐶𝜇 can take.  By default 𝐶𝜇 = 0.09 so: 
0.0009 < 𝐶𝜇 < 0.09 
2.  For the Standard Wilcox 06 𝑘 -𝜔 model, the following two equations are solved for 
the turbulent kinetic energy and the specific turbulent dissipation rate respectively 
𝑘 and 𝜔  : 
𝜕𝑘
𝜕𝑡
+
𝜕(𝑘𝑢𝑖)
𝜕𝑥𝑖
=
𝜕
𝜕𝑥𝑗
[(
+
𝜇𝑡
𝜌 𝜎𝑘1
)
𝜕𝑘
𝜕𝑥𝑗
] + 𝑃𝑘 − 𝛽∗𝑘𝜔 + 𝑆𝑘 
𝜕𝑤
𝜕𝑡
+
𝜕(𝑤𝑢𝑖)
𝜕𝑥𝑖
=
𝜕
𝜕𝑥𝑗
[(
+
𝜇𝑡
𝜌 𝜎𝑤1
)
𝜕𝜖
𝜕𝑥𝑗
] + 𝛾
𝑃𝑘 − 𝛽𝜔2 + 𝜎𝑑𝑋𝑘𝜔2 + 𝑆𝜔
With 𝑃𝑘 the 𝑘 production term and 𝑆𝑘, 𝑆𝜔 are the user defined source terms. 𝑃𝑘, 𝛽∗ and 𝛽 
are expressed as: 
𝑃𝑘 =
𝜇𝑡
𝑆2 
𝛽∗ = 𝛽0
∗𝑓𝛽∗     𝛽 = 𝛽01𝑓𝛽 
𝑓𝛽 =
1 + 85𝑋𝜔
1 + 100𝑋𝜔
  𝑓𝛽∗ = 1.   𝜎𝑑 = {
0.  𝑋𝑘 ≤ 0.
1/8  𝑋𝑘 > 0.
𝑋𝑘 =
𝜔3
𝜕𝑘
𝜕𝑥𝑗
𝜕𝜔
𝜕𝑥𝑗
  𝑋𝜔 = ∣
Ω𝑖𝑗Ω𝑗𝑘S𝑘𝑖
∗𝜔)3 ∣ 
(𝛽0
The turbulent viscosity is then: 
𝜇𝑡 = 𝜌
𝑚𝑎𝑥
⎡
𝜔, 𝐶𝑙√
⎢
⎣
2𝑆𝑖𝑗𝑆𝑖𝑗
∗
𝛽0
⎤
⎥
⎦
For the Standard Wilcox 98 model, the following terms are modified: 
𝑓𝛽 =
1 + 70𝑋𝜔
1 + 80𝑋𝜔
  𝑓𝛽∗ =
{{⎧
{{⎨
⎩
1  𝑋𝑘 ≤ 0.
2   𝑋𝑘 > 0.
1 + 680 𝑋𝑘
1 + 400  𝑋𝑘
  𝜎𝑑 = 0. 
The turbulent viscosity is then: 
𝜇𝑡 = 𝜌
For the Menter SST 2003 model, the following equations are solved: 
𝜕𝑘
𝜕𝑡
+
𝜕(𝑘𝑢𝑖)
𝜕𝑥𝑖
=
𝜕
𝜕𝑥𝑗
[(
+
𝜇𝑡
𝜌 𝜎𝑘
)
𝜕𝑘
𝜕𝑥𝑗
] + 𝑃𝑘 − 𝛽0
∗𝑘𝜔 + 𝑆𝑘 
𝜕𝑤
𝜕𝑡
+
𝜕(𝑤𝑢𝑖)
𝜕𝑥𝑖
=
𝜕
𝜕𝑥𝑗
[(
+
𝜇𝑡
𝜌 𝜎𝑤
)
𝜕𝜖
𝜕𝑥𝑗
] +
𝜇𝑡
𝑃𝑘 − 𝛽𝜔2 + 2(1 − 𝐹1) 𝜎𝑤2𝑋𝑘𝜔2 + 𝑆𝜔 
Each of the constants, 𝛾, 𝛽, 𝜎𝑘, 𝜎𝑤 are now computed by a blend via: 
Where the blending function 𝐹1 is defined by: 
𝛼 = 𝛼1𝐹1 + 𝛼2(1 − 𝐹1)
𝐹1 = tanh ⟨
⎡𝑚𝑖𝑛
⎢
⎣
⎜⎜⎛𝑚𝑎𝑥
⎝
⎜⎜⎛ √𝑘
∗𝜔𝑦
𝛽0
⎝
,
500𝜈
⎟⎟⎞ ,
𝑦2𝜔 ⎠
4𝜌𝜎𝑤2𝑘
𝐶𝐷 𝑦2
⎤
⎥
⎦
⎟⎟⎞
⎠
⟩ 
With 𝑦 the distance to the nearest wall and: 
𝐶𝐷 = 𝑚𝑎𝑥(2𝜌𝜎𝜔2𝑋𝑘𝜔2, 10−10) 
The turbulent viscosity is then: 
𝜇𝑡 = 𝜌
𝑎1𝑘
𝑚𝑎𝑥(𝑎1𝜔, 𝑆 𝐹2)
With: 
𝐹2 = 𝑡𝑎𝑛ℎ
𝑚𝑎𝑥
⎜⎜⎛ 2√𝑘
∗𝜔𝑦
𝛽0
⎝
,
500𝜈
⎟⎟⎞
𝑦2𝜔 ⎠
⎡
⎜⎜⎜⎜⎛
⎢⎢
⎝
⎣
⎟⎟⎟⎟⎞
⎠
⎤
⎥⎥
⎦
3. 
It is possible to activate a limiter on the production term 𝑃𝑘.  If 𝐶𝑐𝑢𝑡 ≥ 0., then : 
𝑃𝑘 = 𝑚𝑖𝑛(𝑃𝑘, 𝐶𝑐𝑢𝑡𝜀)  if  TMOD = 1,  𝑃𝑘 = 𝑚𝑖𝑛(𝑃𝑘, 𝐶𝑐𝑢𝑡𝛽0
especially common when using the Menter SST 2003 model. 
∗𝑘𝜔)  if  TMOD = 4.    This  is 
4.  For RANS models, the following laws of the wall are available : 
a) 
STANDARD CLASSIC : 
𝑈+ =
ln (𝐸 𝑌+) 
If 𝑌+ > 11.225, 𝑈+ = 𝑌+ otherwise 
𝜌𝑦𝑈𝜏
𝑌+ =
𝑈+ =
𝑈𝜏
𝑈𝜏 = √
𝜏𝑤
This is the default for TMOD = 1 
b)  STANDARD LAUNDER and SPALDING :
𝑈∗ =
ln(𝐸 𝑌∗) 
If 𝑌∗ > 11.225, 𝑈∗ = 𝑌∗ otherwise 
𝑌∗ =
𝜌𝐶𝜇
1/4𝑘1/2𝑦
𝑈∗ =
𝑈𝐶𝜇
1/4𝑘1/2
𝑈𝜏
𝑈𝜏 = √
𝜏𝑤
c)  The NON EQUILIBRUM laws of the wall modify the expression of the ve-
locity at the wall making it sensitive to the pressure gradient : 
𝑈 = 𝑈 −
⎡ 𝑦𝑣
𝑑𝑃
⎢
𝑑𝑥 ⎣
𝜌𝜅√𝑘
𝑙𝑛 (
𝑦𝑣
) +
𝑦 − 𝑦𝑣
𝜌𝜅√𝑘
+
𝑦𝑣
⎤ 
⎥
𝜇 ⎦
With: 
𝑦𝑣 =
11.225
𝑦∗
𝑦 
This law is recommended with TMOD = 1 and in cases of complex flows involving 
separation, reattachment and recirculation. 
d)  The automatic wall law attempts to blend the viscous and log layers to bet-
ter account for the transition zone.  In the buffer region, we have : 
𝑈+ =
𝑈𝜏
𝑈𝜏 =
√
√√
⎷
𝑦+)4 + (
(
𝜅 ln (𝐸𝑦+)
)4
This is the recommended approach for TMOD = 4. 
5.  The LES Smagorinsky turbulence model uses the Van Driest damping function 
close to the wall : 
𝑓𝑣 = 1 − 𝑒
−
𝑦+
𝐴+
6.  When a RANS turbulence model is selected, it is possible to define extra parame-
ters to account for the rugosity effects.  In such cases, an extra term will be added 
to the logarithmic part of the different laws of the wall : 
𝑈+ =
ln(𝐸 𝑌+) − Δ𝐵 
If we introduce the non-dimensional roughness height 𝐾+ =
1/4𝑘1/2
𝜌𝐾𝑠𝐶𝜇
, we have: 
Δ𝐵 = 0 𝑓𝑜𝑟 𝐾+ ≤ 2.25 
Δ𝐵 =
𝑙𝑛 [
𝐾+ − 2.25
87.75
+ 𝐶𝑠𝐾+] × 𝑠𝑖𝑛(0.4258(ln 𝐾+ − 0.811)) 𝑓𝑜𝑟 2.25 < 𝐾+ ≤ 90.0 
Δ𝐵 =
𝑙𝑛(1 + 𝐶𝑠𝐾+) 𝑓𝑜𝑟 90. < 𝐾+
*ICFD_CONTROL_TURB_SYNTHESIS 
Purpose:  This keyword enables the user impose a divergence-free turbulent field on inlets.  
Card must be used jointly with VAD = 4 of keyword *ICFD_BOUNDARY_PRESCRIBED_-
VEL. 
  Card 1 
1 
Variable 
PID 
Type 
Default 
I 
0 
2 
IU 
F 
3 
IV 
F 
4 
IW 
F 
5 
LS 
F 
10-3 
10-3 
10-3 
ℎ𝑚𝑖𝑛 
6 
7 
8 
  VARIABLE   
DESCRIPTION 
PID 
Part ID of the surface with the turbulent velocity inlet condition. 
IU, IV, IW 
Intensity of field fluctuations over 𝑥, 𝑦, and 𝑧 directions, 
IU =
𝑢′
𝑢avg
. 
LS 
Integral length scale of turbulence 
Remarks: 
1. 
If  this  card  is  not  defined  but  a  turbulent  field  inlet  has  been  activated.    See 
VAD = 4 of *ICFD_BOUNDARY_PRESCRIBED_VEL, the default parameters will 
be used.
*ICFD 
Purpose:  This keyword enables the computation of time average variables at given time 
intervals. 
2 
3 
4 
5 
6 
7 
8 
DESCRIPTION 
Over  each  DT  time  interval,  an  average  of  the  different  fluid
variables will be calculated and then reset when moving to the next
DT interval. 
  Card 1 
Variable 
1 
DT 
Type 
F 
Default 
none 
  VARIABLE   
DT 
Remarks: 
1.  The file name for this database is icfdavg.*.dat with the different averaged variable 
values copied in a ASCII format.
*ICFD_DATABASE_DRAG_{OPTION}  
Available options include 
VOL 
Purpose:  This keyword enables the computation of drag forces over given surface parts of 
the model.  If multiple keywords are given, the forces over the PID surfaces are given in 
separate files and are also added and output in a separate file. 
For  the  VOL  option,  drag  calculation  can  also  be  applied  on  a  volume  defined  by 
ICFD_PART_VOL.    This  is  mostly  useful  in  porous  media  applications  to  output  the 
pressure drag of the porous media domain. 
Surface Drag Cards.  Include one card for each surface on which drag is applied.  This 
input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
CPID 
DTOUT 
PEROUT 
DIVI 
ELOUT 
SSOUT 
Type 
I 
I 
F 
Default 
none 
none 
0. 
I 
0 
I 
10 
I 
0 
I 
0 
  VARIABLE   
DESCRIPTION 
PID 
CPID 
DTOUT 
PEROUT 
DIVI 
Part ID of the surface where the drag force will be computed. 
Center point ID used for the calculation of the force’s moment.  By
default the reference frame center is used is 𝟎 = (0, 0, 0). 
Time interval to print the output.  If DTOUT is equal to 0.0, then the 
ICFD timestep will be used. 
Outputs the contribution of the different elements on the total drag
in fractions of the total drag in the d3plots. 
Number of drag divisions for PEROUT.  Default is 10 which means
the contributions will be grouped in 10 deciles.  
ELOUT 
Outputs the drag value of each element in the d3plots. 
SSOUT 
Outputs  the  pressure  loads  caused  by  the  fluid  on  each  solid
segment set in keyword format.  FSI needs to be activated.
*ICFD 
1.  The file name for this database is icfdragi for instantaneous drag and icfdraga for 
the drag computed using average values of pressure and velocities. 
2.  The output contains: 
a) 
“Fpx” , “Fpy”, and “Fpz” refer to the three components of the pressure drag 
force 
where 𝑃 is the pressure and 𝐴 the surface area. 
𝐅𝑝 = ∫ 𝑃𝑑𝑨, 
b) 
“Fvx”, “Fxy”, and “Fvz” refer to the three components of the viscous drag 
force 
𝐅𝑣 = ∫ 𝜇
𝜕u
𝜕y
d𝑨. 
where  𝜕u
face area. 
𝜕y is the shear velocity at the wall, 𝜇 is the viscosity and 𝐴 is the sur-
c) 
“Mpx”, “Mpy”, “Mpz”, “Mvx”, “Mvy”, and “Mvz” refer to the three compo-
nents of the pressure and viscous force moments respectively.
*ICFD_DATABASE_FLUX 
Purpose:  This keyword enables the computation of the flow rate and average pressure 
over given parts of the model.  If multiple keywords are given, separate files are output. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
Type 
I 
Default 
none 
  VARIABLE   
DESCRIPTION 
PID 
Part ID of the surface where the flow rates will be computed. 
Remarks: 
1.  The file name for this database is icfd_flux.dat. 
2.  The flux database contains the flow rate through a section, called “output flux”, 
the average pressure, called “Pre-avg”, 
𝛷 = ∑(𝐕𝑖 ⋅ 𝐧𝑖)𝐴𝑖
, 
𝑃avg =
∑ 𝑃𝑖𝐴𝑖
∑ 𝐴𝑖
, 
and the total area, called “Areatot”.
*ICFD 
Purpose:    This  keyword  allows  the  user  to  trigger  the  calculation  of  the  Heat  transfer 
coefficient using different methods and to control the output options. 
  Card 1 
1 
2 
Variable 
OUT 
HTC 
Type 
Default 
I 
0 
I 
0. 
3 
TB 
F 
0. 
4 
5 
6 
7 
8 
OUTDT 
F 
0. 
  VARIABLE   
OUT 
DESCRIPTION 
Determines if the solver should calculate the heat transfer coefficient
and how to output it : 
EQ.0: No HTC calculation 
EQ.1: HTC calculated and output in LSPP as a surface variable.
EQ.2: The solver will also look for FSI boundaries and output the
HTC  value  at  the  solid  nodes  in  an  ASCII  file  called
icfdhtci.dat. 
EQ.3: The solver will also look for FSI boundaries that are part of
SEGMENT_SETS and output the HTC for those segments 
in  an  ASCII  file  called  icfd_convseg.****.key  in  a  format
that can directly read by LS-DYNA for a subsequent pure 
structural thermal analysis. 
HTC 
Determines how the HTC is calculated. 
EQ.0: Automatically  calculated  by  the  solver  based  on  the 
average temperature flowing through the pipe section . 
EQ.1: User imposed value . 
TB 
Value of the bulk temperature if HTC = 1. 
OUTDT 
Output frequency of the HTC in the various ASCII files.  If left to 0., 
the solver will output the HTC at every timestep.
*ICFD_DATABASE_HTC 
1.  The heat transfer coefficient is frequently used in thermal applications to estimate 
the effect of the fluid cooling and it derived from a CFD calculation. 
2.  The heat transfer coefficient is defined as follows: 
ℎ =
𝑇𝑠 − 𝑇𝑏
with 𝑞 the heat flux, 𝑇𝑠 the surface temperature and 𝑇𝑏 the so called “bulk” tem-
perature.  For external aerodynamic applications, this bulk temperature is often 
defined as a constant (ambient or far field conditions, HTC = 1).  However, for 
internal aerodynamic application, this temperature is often defined as an average 
temperature flowing through the pipe section with the flow velocity being used as 
a weighting factor (HTC = 0).
*ICFD 
Purpose:  This keyword enables the computation of the average quantities on surface nodes 
defined in *ICFD_DATABASE_NODOUT.  
2 
3 
4 
5 
6 
7 
8 
  Card 1 
Variable 
Type 
Default 
1 
ON 
I 
0 
  VARIABLE   
DESCRIPTION 
ON 
If equal to 1, the average quantities will be computed. 
Remarks: 
1.  The file name for this database is icfd_nodeavg.dat.
*ICFD_DATABASE_NODOUT 
Purpose:  This keyword enables the output of ICFD data on surface nodes.  For data in the 
fluid volume, it is advised to use points or tracers . 
Output Options Card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OUTLV 
DTOUT 
Type 
Default 
I 
0 
F 
0. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID1 
NID2 
NID3 
NID4 
NID5 
NID6 
NID7 
NID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
OUTLV 
Determines if the output file should be dumped. 
EQ.0:  No output file is generated. 
EQ.1:  The output file is generated. 
DTOUT 
Time interval to print the output.  If DTOUT is equal to 0.0, then the
ICFD timestep will be used. 
NID.. 
Node IDs. 
Remarks: 
1.  The file name for this database is icfd_nodout.dat.
*ICFD 
Purpose:  This keyword enables the computation of the average quantities on point sets 
using the parameters defined in *ICFD_DATABASE_POINTOUT. 
2 
3 
4 
5 
6 
7 
8 
  Card 1 
Variable 
Type 
Default 
1 
ON 
I 
0 
  VARIABLE   
DESCRIPTION 
ON 
If equal to 1, the average quantities will be computed. 
Remarks: 
1.  The file name for this database is icfd_psavg.dat.
*ICFD_DATABASE_POINTOUT 
Purpose:  This keyword enables the output of ICFD data on points.  
Output Options Card. 
  Card 1 
1 
2 
3 
Variable 
PSID 
DTOUT 
PSTYPE 
Type 
Default 
I 
0 
F 
0. 
I 
0 
4 
VX 
F 
0. 
5 
VY 
F 
0. 
6 
VZ 
F 
0. 
7 
8 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
5 
6 
7 
8 
  Card 2 
1 
Variable 
PID 
Type 
I 
2 
X 
F 
3 
Y 
F 
4 
Z 
F 
Default 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
PSID 
Point Set ID. 
DTOUT 
Time interval to print the output.  If DTOUT is equal to 0.0, then the
ICFD timestep will be used. 
PSTYPE 
Point Set type : 
EQ.0: Fixed points. 
EQ.1: Tracer points using prescribed velocity. 
EQ.2:  Tracer points using fluid velocity. 
EQ.3:  Tracer points using mesh velocity.. 
VX, VY, VZ 
Constant velocities to be used when PSTYPE = 1 
PID 
Point ID
VARIABLE   
DESCRIPTION 
X, Y, Z 
Point initial coordinates 
Remarks: 
1.  The file name for this database is icfd_pointout.dat.
*ICFD_DATABASE_RESIDUALS 
Purpose:  This keyword allows the user to output the residuals of the various systems. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
RLVL 
Type 
Default 
I 
0 
  VARIABLE   
DESCRIPTION 
RLVL 
Residual output level : 
EQ.0: No output. 
EQ.1: Only outputs the number of iterations needed for solving
the pressure Poisson equation. 
EQ.2: Outputs  the  number  of  iterations  for  the  momentum,
pressure, mesh movement and temperature equations. 
EQ.3: Also gives the residual for each iteration during the solve
of the momentum, pressure, mesh movement and tempera-
ture equations. 
Remarks: 
1.  The file names for the momentum, pressure, mesh movement and temperature 
equations  are  called  icfd_residuals.moms.dat,  icfd_residuals.pres.dat,  icfd_-
residuals.mmov.dat, and icfd_residuals.temp.dat respectively.
*ICFD 
Purpose:  This keyword enables the computation of the average temperature and the heat 
flux  over  given  parts  of  the  model.    If  multiple  keywords  are  given,  separate  files  are 
output. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
Type 
I 
Default 
none 
  VARIABLE   
PID 
Remarks: 
DESCRIPTION 
Part ID of the surface where the average temperature and heat flux 
will be computed. 
1.  The file name for this database is icfd_thermal.dat. 
2.  Two average temperature are given in the icfd_thermal.dat file: “Temp-avg” and 
“Temp-sum”.  The average temperature is calculated using the local node area as 
weighting factor, 
𝑇avg =
∑ 𝑇𝑖𝐴𝑖
∑ 𝐴𝑖
, 
whereas, the sum is not weighted by area 
𝑇sum =
∑ 𝑇𝑖
If the mesh is regular, the two values will be of similar value.  The icfd_thermal.dat 
output file also includes the average heat flux, the total surface area, and the aver-
age heat transfer coefficients .
*ICFD_DATABASE_TIMESTEP 
Purpose:  This keyword enables the output of ICFD data regarding the ICFD timestep. 
Output Options Card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OUTLV 
Type 
Default 
I 
0 
  VARIABLE   
DESCRIPTION 
OUTLV 
Determines if the output file should be dumped. 
EQ.0:  No output file is generated. 
EQ.1:  The output file is generated. 
Remarks: 
1.  The file name for this database is icfd_tsout.dat.  
2.  Outputs the run’s ICFD timestep versus the timestep calculated using the ICFD 
CFL condition as criteria (autotimestep).  This can be useful in cases using a fixed 
timestep where big mesh deformations and/or big fluid velocity changes occur in 
order  to  track  how  that  fixed  timestep  value  compares  to  the  reference  auto-
timestep.
*ICFD 
Purpose:  This keyword allows the user to have the solver calculate the uniformity index 
. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OUT 
Type 
Default 
I 
0 
  VARIABLE   
DESCRIPTION 
OUT 
Determines if the solver should calculate the uniformity index. 
EQ.0: Off. 
EQ.1: On. 
Remarks: 
1.  Uniformity  Index.    The  uniformity  index  is  a  post  treatment  quantity  which 
measures how uniform the flow is through a given section.  It is especially useful 
in internal aerodynamics cases.  It is expressed as : 
⎡√(𝑢𝑖 − 𝑢̅)2
⎢⎢
𝑢̅
⎣
with 𝐴𝑖, the local cell area, 𝐴 the total section area, 𝑢𝑖 the local velocity, 𝑢̅ the aver-
age velocity through the section, and 𝑛 the number of cells.  
2𝑛𝐴
∑
𝑖=1
𝛾 = 1 −
⎤
⎥⎥
⎦
𝐴𝑖
Values close to 0 means that the flow is very unevenly distributed.  This can be 
used  to  identify  bends,  corners  or  turbulent  effects.    Values  close  to  1  imply 
smooth or equally distributed flow through the surface.
*ICFD_DEFINE_POINT 
Purpose:  This keyword defines a point in space that could be used for multiple purposes. 
5 
6 
7 
8 
  Card 1 
1 
Variable 
POID 
Type 
I 
2 
X 
F 
3 
Y 
F 
4 
Z 
F 
Default 
none 
none 
none 
none 
Optional Card 2. Load curve IDS specifying velocity components of translating point 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
LCIDX 
LCIDY 
LCIDZ 
Type 
Default 
I 
0 
I 
0 
I 
0 
Optional Card 3. Load curve IDS and rotation axis of rotating point 
  Card 2 
1 
Variable 
LCIDW 
Type 
Default 
I 
0 
2 
XT 
F 
3 
YT 
F 
4 
ZT 
F 
5 
XH 
F 
6 
YH 
F 
7 
ZH 
F 
8 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION
POID 
X/Y/Z 
Point ID. 
x, y ,z coordinates for the point.
VARIABLE   
DESCRIPTION
LCIDX/LCIDY/LCIDZ 
The point can be made to translate.  Those are the three
load curve IDs for the three translation components.  
LCIDW 
The  point  can  also  be  made  to  rotate.    This  load  curve
specifies the angular velocity. 
XT/YT/ZT 
Rotation axis tail point coordinates. 
XH/YH/ZH 
Rotation axis head point coordinates. 
.
*ICFD_DEFINE_NONINERTIAL 
Purpose:  This keyword defines a non-inertial reference frame in order to avoid heavy 
mesh distortions and attendant remeshing associated with large-scale rotations.  This is 
used to model, for example, spinning cylinders, wind turbines, and turbo machinery. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
Variable 
1 
W1 
2 
W2 
3 
W3 
Type 
F 
F 
F 
4 
R 
F 
5 
PTID 
I 
6 
L 
F 
7 
8 
LCID 
RELV 
I 
I 
0 
Default 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
W1, W2, W3 
Rotational Velocity along the X,Y,Z axes 
R 
PTID 
Radius of the rotating reference frame 
Starting  point  ID  for  the  reference  frame   
L 
Length of the rotating reference frame 
LCID 
Load curve for scaling factor of w 
→
+
PTID
Figure 5-5.  Non Inertial Reference Frame Example
VARIABLE   
DESCRIPTION 
RELV 
Velocities computed and displayed: 
EQ.0: Relative velocity, only the non-rotating components of the 
velocity are used and displayed. 
EQ.1: Absolute velocity .  All the components of the velocity are
used.  Useful in cases where several or at least one non-
inertial reference frame is combined with an inertial “clas-
sical” reference frame.
*ICFD_DEFINE_WAVE_DAMPING 
Purpose:  This keyword defines a damping zone for free surface waves. 
  Card 1 
1 
Variable 
PID 
2 
NID 
Type 
I 
F 
3 
L 
F 
4 
F1 
F 
5 
F2 
F 
Default 
none 
none 
10 
10 
6 
N 
I 
1 
7 
8 
LCID 
I 
none 
  VARIABLE   
DESCRIPTION
PID 
NID 
L 
F1/F2 
N 
LCID 
.
Point ID defining the start of the damping layer. 
Normal  ID  defined  using  ICFD_DEFINE_POINT  and
pointing to the outgoing direction of the damping layer. 
Length  of  damping  layer.    If  no  is  value  specified,  the
damping  layer  will  have  a  length  corresponding  to  five
element lengths.  
Linear and quadratic damping factor terms. 
Damping term factor. 
Load curve ID acting as temporal scale factor on damping 
term.
*ICFD 
Purpose:  Simple initialization of velocity and temperature within a volume. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
  Card 1 
1 
Variable 
PID 
Type 
I 
2 
Vx 
F 
3 
Vy 
F 
4 
Vz 
F 
5 
T 
F 
6 
P 
F 
7 
8 
Default 
none 
none 
none 
none 
none 
none 
  VARIABLE   
PID 
DESCRIPTION 
Part ID for the volume elements or the surface elements where the 
values  are  initialized  .
PID = 0 to assign the initial condition to all nodes at once. 
Vx 
Vy 
Vz 
T 
P 
x coordinate for the velocity. 
y coordinate for the velocity. 
z coordinate for the velocity. 
Initial temperature. 
Initial Pressure.
*ICFD_INITIAL_TURBULENCE 
Purpose:  When a RANS turbulent model is selected, it is possible to modify the default 
initial values of the turbulent quantities using this keyword. 
Include as many cards as needed.  This input ends at the next keyword (“*”) card. 
4 
5 
6 
7 
8 
  Card 1 
1 
Variable 
PID 
Type 
I 
2 
I 
F 
3 
R 
F 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
Part ID for the volume elements or the surface elements where the 
values  are  initialized  .
PID = 0 to assign the initial condition to all nodes at once. 
Initial turbulent intensity.  
Initial turbulent viscosity to laminar viscosity ratio (𝑟 =
𝜇𝑡𝑢𝑟𝑏
𝜇 ). 
PID 
I 
R 
Remarks: 
1. 
If  no  initial  conditions  have  been  assigned  to  a  specific  PID,  the  solver  will 
automatically pick I = 0.05 (5%) and R = 10000.
Available options include 
TITLE 
*ICFD 
Purpose:  Specify physical properties for the fluid material. 
Fluid Material Card Sets: 
The Material Fluid Parameters Card is required.  If a second card is given, it must be a 
Thermal Fluid Parameters Card.  If the fluid thermal properties are not needed, the second 
card can be a blank card.  In the third card, it is possible to associate the fluid material to a 
Non-Newtonian model and/or to a Porous media model . 
Material Fluid Parameters Card. 
  Card 1 
1 
2 
Variable 
MID 
FLG 
Type 
I 
Default 
none 
I 
1 
3 
RO 
F 
0 
4 
VIS 
F 
0 
5 
ST 
F 
0 
6 
7 
8 
Thermal Fluid Parameters Card. Only to be defined if the thermal problem is solved. 
  Card 2 
Variable 
Type 
Default 
1 
HC 
F 
0 
2 
TC 
F 
0 
3 
4 
5 
6 
7 
8 
BETA 
PRT 
HCSFLCID TCSFLCID 
F 
0 
F 
I 
I 
0.85 
none 
none
Additional fluid models. Only to be defined if the fluid is non-newtonian and/or is a 
porous media. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NNMOID  PMMOID 
Type 
I 
I 
Default 
none 
none 
  VARIABLE   
DESCRIPTION 
MID 
FLG 
RO 
VIS 
ST 
HC 
TC 
BETA 
PRT 
Material ID. 
Flag to choose between fully incompressible, slightly compressible, 
or barotropic flows. 
EQ.0 : Vacuum (free surface problems only) 
EQ.1 : Fully incompressible fluid. 
Flow density. 
Dynamic viscosity. 
Surface tension coefficient. 
Heat capacity.  
Thermal conductivity. 
Thermal expansion coefficient used in the Boussinesq approxima-
tion for buoyancy. 
Turbulent  Prandlt  number.    Only  used  if  K-Epsilon  turbulence 
model selected. 
HCSFLCID 
Load curve ID for scale factor applied on HC function of time.  See 
*DEFINE_CURVE, *DEFINE_CURVE_FUNCTION, or *DEFINE_-
FUNCTION.    If  a  DEFINE_FUNCTION  is  used,  the  following 
parameters are allowed:  𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑡𝑖𝑚𝑒).
Load curve ID for scale factor applied on TC function of time.  See 
*DEFINE_CURVE, *DEFINE_CURVE_FUNCTION, or *DEFINE_-
FUNCTION.    If  a  DEFINE_FUNCTION  is  used,  the  following 
parameters are allowed:  𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑡𝑖𝑚𝑒). 
Non-Newtonian model ID.  This refers to a Non-Newtonian fluid 
model defined using *ICFD_MODEL_NONNEWT. 
Porous  media  model  ID.    This  refers  to  a  porous  media  model
defined using *ICFD_MODEL_POROUS. 
*ICFD_MAT 
  VARIABLE   
TCSFLCID 
NNMOID 
PMMOID 
Remarks: 
1. 
If a K-Epsilon turbulence model is used and the heat transfer equation is solved, 
then the effective thermal conductivity will be determined by : 
𝑘𝑒𝑓𝑓 = 𝑘 +
𝐶𝑝𝜇𝑡𝑢𝑟𝑏
𝑃𝑟𝑡𝑢𝑟𝑏
*ICFD_MODEL_NONNEWT 
Purpose:  Specify a non-newtonian model or a viscosity law that can associated to a fluid 
material. 
Non-Newtonian Model ID and type. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NNMOID 
NNID 
Type 
I 
I 
Default 
none 
none 
Non-Newtonian Fluid Parameters Card.  
  Card 2 
Variable 
Type 
1 
K 
F 
2 
N 
F 
3 
4 
5 
6 
7 
8 
MUMIN 
LAMBDA 
ALPHA 
TALPHA 
F 
F 
F 
F 
Default 
0.0 
0.0 
0.0 
1.e30 
0.0 
0.0 
  VARIABLE   
DESCRIPTION 
NNMOID 
Non-Newtonian Model ID. 
NNID 
Non-Newtonian fluid model type : 
EQ.1 : Power-Law model 
EQ.2 : Carreau model 
EQ.3 : Cross model 
EQ.4 : Herschel-Bulkley model 
EQ.5 : Cross II model 
EQ.6 : Sutherland formula for temperature dependent viscosity
EQ.7 : Power-Law for temperature dependent viscosity 
EQ.8 : Viscosity defined by Load Curve ID or Function ID
VARIABLE   
DESCRIPTION 
K 
N 
MUMIN 
LAMBDA 
Consistency  index  if  NNID = 1  and  4.    Zero  shear  Viscosity  if 
NNID = 2,3 and 5.Reference viscosity if NNID = 6 and NNID = 7. 
Load curve ID or function ID if NNID = 8. 
Measure of the deviation of the fluid from Newtonian (Power Law 
index) for NNID = 1,2,3,4,5,7. Not used for NNID = 6 and 8. 
Minimum  acceptable  viscosity  value  if  NNID = 1.    Infinite  Shear 
Viscosity if NNID = 2,5.Yielding viscosity if NNID = 4.Not used if 
NNID = 3,6,7,8. 
Maximum acceptable viscosity value if NNID = 1.  Time constant if 
NNID = 2,  3,  5.    Yield  Stress  Threshold  if  NNID = 4.Sutherland 
constant if NNID = 6.  Not used if NNID = 7,8. 
ALPHA 
Activation energy if NNID = 1, 2.  Not used if NNID = 3,4,5,6,7,8.
TALPHA 
Reference temperature if NNID = 2.  Not used if NNID = 1,3,4,5,6,7,8
Remarks: 
1.  For the Non-Newtonian models, the viscosity is expressed as : 
a)  POWER-LAW : 
𝜇 = 𝑘𝛾̇ 𝑛−1𝑒𝛼𝑇0 𝑇⁄  
𝜇𝑚𝑖𝑛 < 𝜇 < 𝜇𝑚𝑎𝑥 
With 𝑘 the consistency index, 𝑛 the power law index, 𝛼 the activation energy, 𝑇0 
the initial temperature, 𝑇 the temperature at any given time 𝑡, 𝜇𝑚𝑖𝑛 the mini-
mum acceptable viscosity and 𝜇𝑚𝑎𝑥 the maximum acceptable viscosity. 
b)  CARREAU : 
𝜇 = 𝜇∞ + (𝜇0 − 𝜇∞)[1 + (𝐻(𝑇)𝛾̇𝜆)2](𝑛−1) 2⁄  
𝐻(𝑇) = 𝑒𝑥𝑝 [𝛼(
𝑇 − 𝑇0
−
𝑇𝛼 − 𝑇0
)] 
With 𝜇∞ the infinite shear viscosity, 𝜇0 the zero shear viscosity, 𝑛 the power law 
index, 𝜆 a time constant, 𝛼 the activation energy, 𝑇0 the initial temperature, 𝑇 
the temperature at any given time 𝑡 and 𝑇𝛼 the reference temperature at which 
𝐻(𝑇) = 1.
*ICFD_MODEL_NONNEWT 
𝜇 =
𝜇0
1 + (𝜆𝛾̇)1−𝑛 
With 𝜇0 the zero shear viscosity, 𝑛 the power law index and 𝜆 a time constant. 
d)  HERSCHEL-BULKLEY : 
𝜇 = 𝜇0 𝑖𝑓  (𝛾̇ < 𝜏0 𝜇0⁄
) 
𝜇 =
𝜏0 + 𝑘[𝛾̇ 𝑛 − (𝜏0 𝜇0⁄
)𝑛]
𝛾̇
With 𝑘 the consistency index, 𝜏0 the Yield stress threshold, 𝜇0 the yielding vis-
cosity and 𝑛 the power law index. 
e)  CROSS II : 
𝜇 = 𝜇∞ +
𝜇0 − 𝜇∞
1 + (𝜆𝛾̇)𝑛 
With 𝜇0 the zero shear viscosity, 𝜇∞ the infinite shear viscosity, 𝑛 the power law 
index and 𝜆 a time constant. 
2.  For the temperature dependent viscosity models, the viscosity is expressed as : 
a) 
SUTHERLAND’s LAW : 
𝜇 = 𝜇0(
𝑇0
)3/2 𝑇0 + 𝑆
𝑇 + 𝑆
With 𝜇0 a reference viscosity, 𝑇0 the initial temperature (which therefore must 
not be 0.), 𝑇 the temperature at any given time 𝑡 and 𝑆 Sutherland’s constant. 
b)  POWER LAW : 
𝜇 = 𝜇0(
𝑇0
)𝑛 
With 𝜇0 a reference viscosity, 𝑇0 the initial temperature (which therefore must 
not be 0.), 𝑇 the temperature at any given time 𝑡 and 𝑛 the power law index. 
3.  For NNID = 8, a load curve, a load curve function or a function can be used.  If it 
references  a  DEFINE_FUNCTION,  the  following  arguments  are  allowed 
𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝 , 𝑝𝑟𝑒𝑠, 𝑠ℎ𝑒𝑎𝑟, 𝑡𝑖𝑚𝑒).
Purpose:  Specify a porous media model. 
Porous Media Model ID and type. 
*ICFD 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PMMOID 
PMID 
Type 
I 
I 
Default 
none 
none 
Porous Media Parameters Card.  
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
POR 
PER/THX 
FF/THY 
THZ 
PVLCIDX  PVLCIDY  PVLCIDZ 
Type 
F 
Default 
0. 
F 
0. 
F 
0. 
F 
I 
I 
I 
0. 
none 
none 
none 
Permeability Vector Card in local reference frame. Only to be defined if the porous 
media is anisotropic. 
4 
5 
6 
7 
8 
  Card 3 
1 
Variable 
KX’ 
Type 
F 
Default 
0. 
2 
KY’ 
F 
0. 
3 
KZ’ 
F 
0.
Projection of local Vectors in global reference frame. Only to be defined if the porous 
media is anisotropic. 
  Card 4 
1 
2 
3 
Variable  1-X/1-PID  1-Y/2-PID 
1-Z 
4 
2-X 
5 
2-Y 
6 
2-Z 
7 
8 
Type 
F/I 
F/I 
F/I 
F/I 
F/I 
F/I 
Default 
0 
0. 
0. 
0. 
0. 
0. 
  VARIABLE   
DESCRIPTION 
PMMOID 
Porous media model ID. 
PMID 
Porous media model type : 
EQ.1 : Isotropic porous media - Ergun Correlation. 
EQ.2 : Isotropic porous media - Darcy-Forchheimer model. 
EQ.3 : Isotropic  porous  media  -  Permeability  defined  through 
Pressure-Velocity Data. 
EQ.4 : Anisotropic  porous  media  -  Fixed  local  reference  frame 
. 
EQ.5 : Anisotropic porous media model - Moving local reference 
frame  and  permeability  vector  in  local  reference  frame 
(𝑥’, 𝑦’, 𝑧’)  defined by three Pressure-Velocity curves. 
EQ.6 : Anisotropic porous media model - Moving local reference 
frame and permeability vector constant. 
EQ.7:  Anisotropic porous media model - Moving local reference 
frame and permeability vector constant.  This model dif-
fers from PMID = 6 in the way the local reference frame is 
moved. 
POR 
Porosity 𝜀. 
PER/THX 
FF/THY 
Permeability 𝜅 if PMID = 1 or 2.  Probe Thickness ∆𝑥 if PMID = 3 or 
PMID = 5. 
Forchheimer factor.  To Be defined if PMID = 2. Probe Thickness ∆𝑦
if PMID = 5. 
THZ 
Probe Thickness ∆𝑧 if PMID = 5.
DESCRIPTION 
Pressure  function  of  Velocity  Load  Curve  ID.    To  be  defined  if 
PMID = 3  and  PMID = 5.  If  PMID = 5,  this  refers  to  P-V  curve  in 
global X direction. For PMID = 1 and PMID = 2, this flags acts as an 
optional load curve ID, define curve function ID or define function
ID.  If a DEFINE_FUNCTION is used, the following parameters are
allowed:  𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑡𝑖𝑚𝑒).     
Pressure  function  of  Velocity  Load  Curve  ID.    To  be  defined  if 
PMID = 5.  This refers to P-V curve in global Y direction.  
Pressure  function  of  Velocity  Load  Curve  ID.    To  be  defined  if 
PMID = 5.  This refers to P-V curve in global Z direction. 
Permeability vector in local reference frame (𝑥’, 𝑦’, 𝑧’).  To be defined 
in  PMID = 4,  5,  6  or  7.    Those  values  become  scale  factors  if 
PMID = 5. 
Projection of local permeability vector 𝐱’ in global reference frame 
(𝑥, 𝑦, 𝑧).  To be defined if PMID = 4. If PMID = 6, those become load 
curve IDs so the coordinates of the local 𝐱’ vector can be made to 
move through time. 
Projection of local permeability vector 𝐲’ in global reference frame 
(𝑥, 𝑦, 𝑧).  To be defined if PMID = 4. If PMID = 6, those become load 
curve IDs so the coordinates of the local 𝐲’ vector can be made to 
move through time. 
If PMID = 5 or PMID = 7, the two local reference frame vectors are 
defined by the coordinates of the two point IDs defined by 1-PID 
and 2-PID.  .  Since those points can be 
made to move, it is therefore possible to define a moving reference
frame for the anisotropic porous media domain. 
  VARIABLE   
PVLCIDX 
PVLCIDY 
PVLCIDZ 
KX’/KY’/KZ’ 
1-X/1-Y/1-Z 
2-X/2-Y/2-Z 
1-PID/2-PID 
Remarks: 
1.  Being 𝜀 the porosity and 𝜅 the permeability of the porous media respectively, one 
can define: 
𝜀 =
𝑣𝑜𝑖𝑑 𝑣𝑜𝑙𝑢𝑚𝑒
𝑡𝑜𝑡𝑎𝑙 𝑣𝑜𝑙𝑢𝑚𝑒
And being 𝑢𝑖 the volume averaged velocity field defined in terms of the fluid ve-
locity field 𝑢𝑖𝑓  as:
y'
x'
Figure 5-6.  Anisotropic porous media vectors definition (PMID = 4,5,6,7).  The
vectors  𝐗    and  𝐘  are  the  global  axes;  𝐱′  and  𝐲′  define  system  for  the  primed
coordinate(𝑥′, 𝑦′, 𝑧′). 
𝑢𝑖 = 𝜀𝑢𝑖𝑓  
The generalized flow equations of momentum and mass conservation can be ex-
pressed as :  
𝜕𝑢𝑖
𝜕𝑥𝑖
= 0 
𝜀 [
𝜕𝑢𝑖
𝜕𝑡 + 𝜕
𝜕𝑥𝑗
𝜕𝑢𝑖𝑢𝑗
𝜀 )] = − 1
(
𝜕(𝑃𝜀)
𝜕𝑥𝑖
+
𝜀 (
𝜕2𝑢𝑖
𝜕𝑥𝑗𝜕𝑥𝑗
) + 𝜌𝑔𝑖 − 𝐷𝑖 
Where 𝐷𝑖 are the forces exerted to the fluid by the porous matrix.  For the isotropic 
model, the porous forces are a function of the matrix porosity and its permeability.  
For the isotropic case, three models are available : 
a)  Model 1 : Ergun correlation 𝐷𝑖 =
b)  Model 2 : Darcy-Forcheimer 𝐷𝑖 =
𝜇𝑢𝑖
𝜅 +
1.75𝜌|𝑈|
√150√𝜅𝜀3/2
𝑢𝑖 
𝜇𝑢𝑖
𝜅 +
𝐹𝜀𝜌|𝑈|
√𝜅
𝑢𝑖 
c)  Model 3 : Using the 𝛥𝑃 − 𝑉 experimental data.  In this case, it is assumed 
that the pressure velocity curve was obtained applying a pressure differ-
ence or pressure drop on both ends of a porous slab of thickness 𝛥𝑥 with 
porous properties 𝜅 and 𝜀.  It then becomes possible for the solver to fit that 
experimental  curve  with  a  quadratic  polynomial  of  the  form  𝛥𝑃(𝑢𝑥) =
𝛼𝑢𝑥
2 + 𝛽𝑢𝑥.  Once 𝛼 and 𝛽 are known, it is possible to estimate 𝐷𝑖. 
2.  The  anisotropic    version  of  the  Darcy-Forcheimer  term  can  be 
written as :
𝐷𝑖 = 𝜇𝐵𝑖𝑗𝜇𝑗 + 𝐹𝜀|𝑈|𝐶𝑖𝑗𝑢𝑗 
𝐵𝑖𝑗 = (𝐾𝑖𝑗)
−1
𝐶𝑖𝑗 = (𝐾𝑖𝑗)
−1/2
Where 𝐾𝑖𝑗 is the anisotropic permeability tensor.
Available options include 
TITLE 
*ICFD_PART 
Purpose:  Define parts for this incompressible flow solver. 
The TITLE option allows the user to define an additional optional line with a HEADING in 
order to associate a name to the part. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
HEADING 
A 
none 
Part  Material  Card.  Include  as  many  cards  as  needed.    This  input  ends  at  the  next 
keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
SECID 
MID 
Type 
I 
I 
I 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
PID 
Part identifier for fluid surfaces. 
SECID 
Section identifier defined with the *ICFD_SECTION card. 
MID 
Material identifier defined with the *ICFD_MAT card.
Available options include 
TITLE 
*ICFD 
Purpose:  This keyword assigns material properties to the nodes enclosed by surface ICFD 
parts. 
The TITLE option allows the user to define an additional optional line with a HEADING in 
order to associate a name to the part. 
Title 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
Default 
HEADING 
A 
none 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
SECID 
MID 
Type 
I 
I 
I 
Default 
none 
none 
none 
Provide as many cards as necessary.  This input ends at the next keyword (“*”) card 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SPID1 
SPID2 
SPID3 
SPID4 
SPID5 
SPID6 
SPID7 
SPID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none
*ICFD_PART_VOL 
DESCRIPTION 
PID 
Part identifier for fluid volumes. 
SECID 
Section identifier defined by the *ICFD_SECTION card. 
MID 
Material identifier. 
SPID1, … 
Part IDs for the surface elements that define the volume mesh. 
PID 3
PID 4
PID 5
PID 3
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$$$$  *ICFD_PART_VOL 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$ PART ID 5 is defined by the surfaces that enclose it. 
$ 
*ICFD_PART_VOL 
$ 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      pid       secid       mid 
        5          1          1 
$...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 
$      pid1      pid2      pid3      pid4      pid5      pid6      pid7      pid8 
         1         2         3         4
*ICFD 
Purpose:  Define a section for the incompressible flow solver. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SID 
Type 
I 
Default 
none 
  VARIABLE   
DESCRIPTION 
SID 
Section identifier.
*ICFD_SET_NODE_LIST 
Purpose:    Only  used  in  cases  where  the  mesh  is  specified  by  the  user  .    Defines  a  set  of  nodes  associated  with  a  part  ID  on  which 
boundary conditions can be applied. 
3 
4 
5 
6 
7 
8 
  Card 1 
1 
Variable 
SID 
2 
PID 
Type 
I 
I 
Default 
none 
none 
Node List Card. Provide as many cards as necessary.  This input ends at the next keyword 
(“*”) card 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NID1 
NID2 
NID3 
NID4 
NID5 
NID6 
NID7 
NID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
SID 
PID 
Set ID 
Associated Part ID.  
NID1, … 
Node IDs 
Remarks: 
1.  The convention is the similar to the one used by the keyword *SET_NODE_LIST 
and serves a similar purpose.
*ICFD 
Purpose:  This keyword provides an option to trigger an iterative procedure on the fluid 
system.  This procedure aims to bring more precision to the final pressure and velocity 
values but is often very time consuming.  It must therefore be used with caution.  It is 
intended only for special cases.  For stability purposes, this method is automatically used 
for the first ICFD time step. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
NIT 
TOL 
Type 
Default 
I 
1 
F 
10-3 
  VARIABLE   
DESCRIPTION 
NIT 
TOL 
Maximum Number of iterations of the system for each fluid time
step.  If TOL criteria is not reached after NIT iterations, the run will
proceed. 
Tolerance Criteria for the pressure residual during the fluid system 
solve.
*ICFD_SOLVER_TOL_MMOV 
Purpose:  This keyword allows the user to change the default tolerance values for the mesh 
movement algorithm. Care should be taken when deviating from the default values. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ATOL 
RTOL 
MAXIT 
Type 
F 
F 
I 
Default 
1e-8 
1e-8 
1000 
  VARIABLE   
ATOL 
RTOL 
MAXIT 
DESCRIPTION 
Absolute  convergence  criteria.    Convergence  is  achieved  when
Residual𝑖+1 − Residual𝑖 ≤ ATOL.  If a negative integer is entered, 
then that value will be used as a load curve ID for ATOL. 
Relative  convergence  criteria.    Convergence  is  achieved  when
(Residual𝑖+1 − Residual𝑖) Residualinitial
≤ RTOL.    If  a  negative 
integer is entered, then that value will be used as a load curve ID for 
RTOL. 
⁄
Maximum number of iterations allowed to achieve convergence.  If a
negative integer is entered, then that value will be used as a load
curve ID for MAXIT.
*ICFD 
Purpose:    This  keyword  allows  the  user  to change  the  default  tolerance  values  for  the 
momentum equation solve. Care should be taken when deviating from the default values. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ATOL 
RTOL 
MAXIT 
Type 
F 
F 
I 
Default 
10-8 
10-8 
1000 
  VARIABLE   
ATOL 
RTOL 
MAXIT 
DESCRIPTION 
Absolute  convergence  criteria.    Convergence  is  achieved  when
Residual𝑖+1 − Residual𝑖 ≤ ATOL.  If a negative integer is entered, 
then that value will be used as a load curve ID for ATOL. 
Relative  convergence  criteria.    Convergence  is  achieved  when
(Residual𝑖+1 − Residual𝑖) Residualinitial
≤ RTOL.    If  a  negative 
integer is entered, then that value will be used as a load curve ID for 
RTOL. 
⁄
Maximum number of iterations allowed to achieve convergence.  If a
negative integer is entered, then that value will be used as a load
curve ID for MAXIT.
*ICFD_SOLVER_TOL_MONOLITHIC 
Purpose:    This  keyword  allows  the  user  to change  the  default  tolerance  values  for  the 
monolithic solver. Care should be taken when deviating from the default values. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ATOL 
RTOL 
MAXIT 
Type 
F 
F 
I 
Default 
10-8 
10-8 
1000 
  VARIABLE   
ATOL 
RTOL 
MAXIT 
DESCRIPTION 
Absolute  convergence  criteria.    Convergence  is  achieved  when
Residual𝑖+1 − Residual𝑖 ≤ ATOL.  If a negative integer is entered, 
then that value will be used as a load curve ID for ATOL. 
Relative  convergence  criteria.    Convergence  is  achieved  when
(Residual𝑖+1 − Residual𝑖) Residualinitial
≤ RTOL.    If  a  negative 
integer is entered, then that value will be used as a load curve ID for 
RTOL. 
⁄
Maximum number of iterations allowed to achieve convergence.  If a
negative integer is entered, then that value will be used as a load
curve ID for MAXIT.
*ICFD 
Purpose:    This  keyword  allows  the  user  to change  the  default  tolerance  values  for  the 
Poisson equation for pressure.  Care should be taken when deviating from the default values. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ATOL 
RTOL 
MAXIT 
Type 
F 
F 
I 
Default 
10-8 
10-8 
1000 
  VARIABLE   
ATOL 
RTOL 
MAXIT 
DESCRIPTION 
Absolute  convergence  criteria.    Convergence  is  achieved  when
Residual𝑖+1 − Residual𝑖 ≤ ATOL.  If a negative integer is entered, 
then that value will be used as a load curve ID for ATOL. 
Relative  convergence  criteria.    Convergence  is  achieved  when
(Residual𝑖+1 − Residual𝑖) Residualinitial
≤ 𝑅𝑇𝑂𝐿.    If  a  negative 
integer is entered, then that value will be used as a load curve ID for 
RTOL. 
⁄
Maximum number of iterations allowed to achieve convergence.  If a
negative integer is entered, then that value will be used as a load
curve ID for MAXIT.
*ICFD_SOLVER_TOL_TEMP 
Purpose:  This keyword allows the user to change the default tolerance values for the heat 
equation.  To be handled with great care. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
ATOL 
RTOL 
MAXIT 
Type 
F 
F 
I 
Default 
1e-8 
1e-8 
1000 
  VARIABLE   
ATOL 
RTOL 
MAXIT 
DESCRIPTION 
Absolute  convergence  criteria.    Convergence  is  achieved  when
𝑅𝑒𝑠𝑖𝑑𝑢𝑎𝑙𝑖+1 − 𝑅𝑒𝑠𝑖𝑑𝑢𝑎𝑙𝑖 ≤ 𝐴𝑇𝑂𝐿.  If a negative integer is entered, then 
that value will be used as a load curve ID for ATOL. 
Relative  convergence  criteria.    Convergence  is  achieved  when
(𝑅𝑒𝑠𝑖𝑑𝑢𝑎𝑙𝑖+1 − 𝑅𝑒𝑠𝑖𝑑𝑢𝑎𝑙𝑖) 𝑅𝑒𝑠𝑖𝑑𝑢𝑎𝑙𝑖𝑛𝑖𝑡𝑖𝑎𝑙
≤ 𝑅𝑇𝑂𝐿.  If a negative integer 
is entered, then that value will be used as a load curve ID for RTOL.
⁄
Maximum number of iterations allowed to achieve convergence.  If a
negative integer is entered, then that value will be used as a load
curve ID for MAXIT.
*MESH 
The keyword *MESH is used to create a mesh that will be used in the analysis.  So far only 
tetrahedral (or triangular in 2-d) elements can be generated.  The keyword cards in this 
section are defined in alphabetical order: 
*MESH_BL 
*MESH_BL_SYM 
*MESH_EMBEDSHELL 
*MESH_INTERF 
*MESH_NODE 
*MESH_SIZE 
*MESH_SIZE_SHAPE 
*MESH_SURFACE_ELEMENT 
*MESH_SURFACE_NODE 
*MESH_VOLUME 
*MESH_VOLUME_ELEMENT 
*MESH_VOLUME_NODE 
*MESH_VOLUME_PART 
An additional option “_TITLE” may be appended to all *MESH keywords.  If this option is 
used, then an 80 character string is read as a title from the first card of that keyword's 
input.  At present, LS-DYNA does not make use of the title.  Inclusion of titles gives greater 
clarity to input decks.
*MESH_BL 
Purpose:    This  keyword  is  used  to  define  a  boundary-layer  mesh  as  a  refinement  on 
volume-mesh.  The boundary layer mesh is constructed by subdividing elements near the 
surface. 
Boundary  Layer  Cards.    Define  as  many  cards  as  are  necessary.    The  next  “*”  card 
terminates the input. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID 
NELTH 
BLTH 
BLFE 
BLST 
Type 
I 
I 
F 
Default 
none 
none 
0. 
F 
0. 
I 
0 
  VARIABLE   
DESCRIPTION 
PID 
Part identifier for the surface element. 
NELTH 
BLTH 
BLFE 
Number of elements normal to the surface (in the boundary layer) is 
NELTH+1. 
Boundary layer mesh thickness if BLST = 1 or BLST = 2.  Growth 
scale factor if BLST = 3.  Ignored if BLST = 0. 
Distance between the wall and the first volume mesh node.  Not
used if BLST = 0 or BLST = 1. 
BLST 
Boundary layer mesh generation strategy : 
EQ.0: By  default,  for  every  additional  NELTH,  the  automatic
volume mesher will divide the elements closest to the sur-
face by two so that the smallest element in the boundary
layer mesh will have an aspect ratio of 2NELTH+1.  A default 
boundary layer mesh thickness based on the surface mesh 
size will be chosen. 
EQ.1: Constant repartition using BLFE and NELTH. 
EQ.2: Repartition following a quadratic polynomial. 
EQ.3: Repartition following a growth scale factor.
*MESH 
1.  For BLST = 1, the distance between the wall and the first node will be equal to 
𝐵𝐿𝑇𝐻 (𝑁𝐸𝐿𝑇𝐻 + 1)
⁄
. 
2.  For  BLST = 3,  the  total  thickness  of  the  boundary  layer  will  be  equal  to 
∑
𝑁𝐸𝐿𝑇𝐻
𝑛=0
𝐵𝐿𝐹𝐸  × 𝐵𝐿𝑇𝐻𝑛
.
*MESH_BL_SYM 
Purpose:  Specify the part IDs that will have symmetry conditions for the boundary layer.  
On these surfaces, the boundary layer mesh follows the surface tangent.  
Boundary Layer with Symmetry Condition Cards. Define as many cards as necessary. 
The next “*” card terminates the input. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID1 
PID2 
PID3 
PID4 
PID5 
PID6 
PID7 
PID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
PID1, … 
DESCRIPTION 
Part  identifiers  for  the  surface  element.    This  is  the  surface  with
symmetry.
*MESH 
Purpose:    Define  surfaces  that  the  mesher  will  embed  inside  the  volume  mesh.    These 
surfaces will have no thickness and will conform to the rest of the volume mesh having 
matching nodes on the interface.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VOLID 
Type 
I 
Default 
none 
Define as many cards as are necessary based on the number of PIDs (the next “*” card 
terminates the input.) 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID1 
PID2 
PID3 
PID4 
PID5 
PID6 
PID7 
PID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
VOLID 
PIDn 
ID assigned to the new volume in the keyword *MESH_VOLUME. 
The surface mesh size will be applied to this volume. 
Part  IDs  for  the  surface  elements  that  will  be  embedded  in  the
volume mesh.
*MESH_INTERF 
Purpose:  Define the surfaces that will be used by the mesher to specify fluid interfaces in 
multi-fluid simulations.  
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VOLID 
Type 
I 
Default 
none 
Define as many cards as are necessary based on the number of PIDs.  This input ends at the 
next keyword (“*”) card. 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID1 
PID2 
PID3 
PID4 
PID5 
PID6 
PID7 
PID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
VOLID 
DESCRIPTION 
ID assigned to the new volume in the keyword *MESH_VOLUME. 
The interface meshes will be applied to this volume. 
PIDn 
Part IDs for the surface elements.
*MESH 
Purpose:    Define  a  fluid  node  and  its  coordinates.    These  nodes  are  used  in  the  mesh 
generation  process  by  the  *MESH_SURFACE_ELEMENT  keyword,  or  as  user  defined 
volume nodes by the *MESH_VOLUME_ELEMENT keyword. 
Node  Cards.    Include  one  additional  card  for  each node.   This  input  ends  at  the  next 
keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
NID 
Type 
I 
Default 
none 
X 
F 
0 
Y 
F 
0 
Z 
F 
0 
  VARIABLE   
DESCRIPTION 
NID 
Node ID.  A unique number with respect to the other surface nodes.
X 
Y 
Z 
𝑥 coordinate. 
𝑦 coordinate. 
𝑧 coordinate. 
Remarks: 
1.  The data card format for the *MESH_NODE keyword is identical to *NODE. 
2.  The *MESH_NODE keyword supersedes *MESH_SURFACE_NODE, which was 
for surfaces nodes as well as *MESH_VOLUME_NODE for, which was for volume 
nodes in user defined.
*MESH_SIZE 
Purpose:  Define the surfaces that will be used by the mesher to specify a local mesh size 
inside the volume.  If no internal mesh is used to specify the size, the mesher will use a 
linear interpolation of the surface sizes that define the volume enclosure. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VOLID 
Type 
I 
Default 
none 
Define as many cards as are necessary based on the number of PIDs (the next “*” card 
terminates the input.). 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID1 
PID2 
PID3 
PID4 
PID5 
PID6 
PID7 
PID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
VOLID 
PIDn 
ID assigned to the new volume in the keyword *MESH_VOLUME. 
The mesh sizing will be applied to this volume. 
Part IDs for the surface elements that are used to define the mesh
size next to the surface mesh.
*MESH 
Purpose:  Defines a local mesh size in specific zones corresponding to given geometrical 
shapes (box, sphere, and cylinder).  The solver will automatically apply the conditions 
specified during the generation of the volume mesh.  This zone does not need to be entirely 
defined in the volume mesh.  
Remeshing Control Card sets: 
Add as many remeshing control cards paired with a case card as desired.  The input of such 
pairs ends at the next keyword “*” card. 
Remeshing Control. First card specifies whether to maintain this mesh sizing criterion 
through a remesh operation. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SNAME 
FORCE 
Type 
A 
Default 
none 
I 
0 
Box Case. Card 2 for SNAME = “box” 
  Cards 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MSIZE 
PMINX 
PMINY 
PMINZ 
PMAXX 
PMAXY 
PMAXZ 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none
Sphere Case. Card 2 for SNAME = “sphere” 
  Cards 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MSIZE 
RADIUS  CENTERX CENTERY CENTERZ
Type 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
Cylinder Case. Card 2 for SNAME = “cylinder” 
  Cards 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
MSIZE 
RADIUS 
PMINX 
PMINY 
PMINZ 
PMAXX 
PMAXY 
PMAXZ 
Type 
F 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
SNAME 
DESCRIPTION
Shape  name.    Possibilities  include  “box”,  “cylinder”  and
“sphere” 
FORCE 
Force to keep the mesh size criteria even after a remeshing is
done. 
EQ.0: Off, mesh size shape will be lost if a remeshing occurs
EQ.1: On. 
MSIZE 
Mesh  size  that  needs  to  be  applied  in  the  zone  of  the  shape
defined by SNAME 
PMIN[X, Y, Z] 
𝑥, 𝑦, or 𝑧 value for the point of minimum coordinates 
PMAX[X, Y, Z] 
𝑥, 𝑦, or 𝑧 value for the point of maximum coordinates 
CENTER[X, Y, Z] 
Coordinates  of  the  sphere  center  in  cases  where  SNAME  is
sphere 
RADIUS 
Radius of the sphere if SNAME is Sphere or of the cross section
disk if SNAME is Cylinder.
*MESH 
Purpose:  Specify a set of surface elements (quadrilateral or triangular in 3-d and linear 
segments  in  2-d)  that  will  be  used  by  the  mesher  to  construct  a  volume  mesh.    These 
surface elements may be used to define the enclosed volume to be meshed, or alternatively 
they could be used to apply different mesh sizes inside the volume . 
Surface Element Card. Define as many cards as necessary.  The next “*” card terminates 
the input. 
  Card 1 
1 
2 
Variable 
EID 
PID 
3 
N1 
4 
N2 
5 
N3 
6 
N4 
7 
8 
9 
10 
Type 
I 
I 
I 
I 
I 
I 
Default 
none  none  none  none  none  none 
  VARIABLE   
DESCRIPTION 
Element  ID.    A  unique  number  with  respect  to  all  *MESH_SUR-
FACE_ELEMENTS cards. 
Mesh surface part ID.  A unique identifier for the surface to which 
this mesh surface element belongs. 
Nodal point 1. 
Nodal point 2. 
Nodal point 3. 
Nodal point 4. 
EID 
PID 
N1 
N2 
N3 
N4 
Remarks: 
1.  The convention is the same used by the keyword *ELEMENT_SHELL.  In the case 
of a triangular face N3 = N4.  In 2-d N2 = N3 = N4.  Note that the accepted card 
format is 6i8 (not 6i10)
*MESH_SURFACE_NODE 
Purpose:    Define  a  node  and  its  coordinates.    These  nodes  will  be  used  in  the  mesh 
generation process by the *MESH_SURFACE_ELEMENT keyword.  
*MESH_NODE supersedes this card; so please use *MESH_NODE instead of this card. 
Surface Node Cards.  Include one card for each node.  Include as many cards a necessary. 
This input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
NID 
Type 
I 
Default 
none 
X 
F 
0 
Y 
F 
0 
Z 
F 
0 
  VARIABLE   
DESCRIPTION 
NID 
Node ID.  This NID must be unique within the set of surface nodes.
X 
Y 
Z 
𝑥 coordinate. 
𝑦 coordinate. 
𝑧 coordinate.
*MESH 
Purpose:  This keyword defines the volume space that will be meshed.  The boundaries of 
the volume are the surfaces defined by *MESH_SURFACE_ELEMENT.  The surfaces listed 
have to be non-overlapping, and should not leave any gaps or open spaces between the 
surface boundaries.  On the boundary between two neighbor surfaces, nodes have to be in 
common (no duplicate nodes) and should match exactly on the interface.  They are defined 
by the keyword *MESH_SURFACE_NODE.  This card will be ignored if the volume mesh 
is specified by the user and not generated automatically. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VOLID 
Type 
I 
Default 
none 
Define as many cards as are necessary based on the number of PIDs (the next “*” card 
terminates the input.)
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PID1 
PID2 
PID3 
PID4 
PID5 
PID6 
PID7 
PID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
VOLID 
ID assigned to the new volume. 
PIDn 
Part IDs for the surface elements that are used to define the volume.
*MESH_VOLUME_ELEMENT 
Purpose:  Specify a set of volume elements for the fluid volume mesh in cases where the 
volume mesh is specified by the user and not generated automatically.  The nodal point are 
specified  in  the  *MESH_VOLUME_NODE  keyword.    Only  tetrahedral  elements  are 
supported (triangles in 2D). 
Volume Element Card. Define as many cards as necessary.  The next “*” card terminates 
the input. 
  Card 1 
1 
2 
Variable 
EID 
PID 
3 
N1 
4 
N2 
5 
N3 
6 
N4 
7 
8 
9 
10 
Type 
I 
I 
I 
I 
I 
I 
Default 
none  none  none  none  none  none 
  VARIABLE   
DESCRIPTION 
Element  ID.    A  unique  number  with  respect  to  all  *MESH_VOL-
UME_ELEMENTS cards. 
Part ID.  A unique part identification number. 
Nodal point 1. 
Nodal point 2. 
Nodal point 3. 
Nodal point 4. 
EID 
PID 
N1 
N2 
N3 
N4 
Remarks: 
1.  The convention is the same used by the keyword *ELEMENT_SOLID.
*MESH 
Purpose:  Define a node and its coordinates.  This keyword is only used in cases where the 
fluid volume mesh is provided by the user and is not automatically generated.  It serves the 
same purpose as the *NODE keyword for solid mechanics.  Only tetrahedral elements are 
supported.  
*MESH_NODE supersedes this card; so please use *MESH_NODE instead of this card. 
Volume Node Cards. Include as many cards in the following format as desired.  This input 
ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
9 
10 
Variable 
NID 
Type 
I 
Default 
none 
X 
F 
0 
Y 
F 
0 
Z 
F 
0 
  VARIABLE   
DESCRIPTION 
NID 
Node ID.  A unique number with respect to the other volume nodes.
X 
Y 
Z 
𝑥 coordinate. 
𝑦 coordinate. 
𝑧 coordinate.
*MESH_VOLUME_PART 
Purpose:  Associate a volume part number created by a *MESH_VOLUME card with the 
part number of a part card from a selected solver (designated by the SOLVER field). 
Mesh Volume Part Card. Include as many cards in the following format as desired.  This 
input ends at the next keyword (“*”) card. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
VOLPRT 
SOLPRT 
SOLVER 
Type 
I 
I 
A 
Default 
  VARIABLE   
DESCRIPTION 
VOLPRT 
Part ID of a volume part created by a *MESH_VOLUME card. 
SOLPRT 
Part ID of a part created using SOLVER’s part card. 
SOLVER 
Name of a solver using a mesh created with *MESH cards.
*STOCHASTIC 
The keyword *STOCHASTIC is used to describe the particles and numerical details for 
solving a set of stochastic PDEs.  Currently, there are two types of stochastic PDE models in 
the code: a  model of embedded particles in TBX explosives, and a spray model.  The cards 
for using these models are: 
*STOCHASTIC_SPRAY_PARTICLES 
*STOCHASTIC_TBX_PARTICLES 
An additional option “_TITLE” may be appended to all *STOCHASTIC keywords.  If this 
option  is  used,  then  an  80  character  string  is  read  as  a  title  from  the  first  card  of  that 
keyword's input.  At present, LS-DYNA does not make use of the title.  Inclusion of titles 
gives greater clarity to input decks.
*STOCHASTIC_SPRAY_PARTICLES 
Purpose:  Specify particle and other model details for spray modeling using stochastic 
PDEs  that  approximate  such  processes.    A  pair  of  cards  is  required  to  specify  the 
characteristics of each nozzle (cards 3 and 4 describe the first nozzle). 
Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
INJDIST 
IBRKUP 
ICOLLDE 
IEVAP 
IPULSE 
LIMPR 
IDFUEL 
Type 
Default 
I 
1 
I 
I 
none 
none 
Card 2 
1 
2 
3 
I 
0 
4 
I 
I 
none 
none 
5 
6 
I 
1 
7 
8 
Variable 
RHOP 
TIP 
PMASS 
PRTRTE 
STRINJ 
DURINJ 
Type 
F 
F 
F 
F 
F 
F 
Nozzle card 1: Provide as many pairs of nozzle cards 1 and 2 as necessary.  This input 
ends at the next keyword (“*”) card (following a nozzle card 2). 
Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
XORIG 
YORIG 
ZORIG 
SMR 
VELINJ 
DRNOZ 
DTHNOZ 
Type 
F 
F 
F 
F 
F 
F
Nozzle card 2: Provide as many pairs of nozzle cards 1 and 2 as necessary.  This input 
ends at the next keyword (“*”) card. 
Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
TILTXY 
TILTXZ 
CONE 
DCONE 
ANOZ 
AMP0 
Type 
F 
F 
F 
F 
F 
F 
  VARIABLE   
DESCRIPTION 
INJDIST 
Spray particle size distribution: 
EQ.1: 
EQ.2: 
EQ.3: 
EQ.4: 
uniform 
Rosin-Rammler (default) 
Chi-squared degree of 2 
Chi-squared degree of 6 
IBRKUP 
Type of particle breakup model: 
EQ.0: 
EQ.1: 
EQ.2: 
off (no breakup) 
TAB 
KHRT 
ICOLLDE 
Turn collision modeling on or off 
IEVAP 
Evaporation flag: 
EQ.0: 
EQ.1: 
off (no evaporation) 
Turn evaporation on  
IPULSE 
Type of injection: 
EQ.0: 
EQ.1: 
EQ.2: 
continuous injection 
sine wave 
square wave 
LIMPRT 
Upper limit on the number of parent particles modeled in this spray.
This is not used with the continuous injection case (IPULSE = 0).
VARIABLE   
DESCRIPTION 
IDFUEL 
Selected spray liquid fuels: 
EQ.1: 
EQ.2: 
EQ.3: 
EQ.4: 
EQ.5: 
EQ.6: 
EQ.7: 
EQ.8: 
EQ.9: 
(Default), H2O 
Benzene, C6H6 
Diesel # 2, C12H26 
Diesel # 2, C13H13 
Ethanol, C2H5OH 
Gasoline, C8H18 
Jet-A, C12H23 
Kerosene, C12H23 
Methanol, CH3OH 
EQ.10: 
N-dodecane, C12H26 
RHOP 
Particle density 
TIP 
Initial particle temperature. 
PMASS 
Total particle mass 
PRTRTE 
Number of particles injected per second for continuous injection. 
STRINJ 
Start of injection(s) 
DURINJ 
Duration of injection(s) 
XORIG 
X-coordinate of center of a nozzle’s exit plane 
YORIG 
Y-coordinate of center of a nozzle’s exit plane 
ZORIG 
Z-coordinate of center of a nozzle’s exit plane 
SMR 
Sauter mean radius 
VELINJ 
Injection velocity 
DRNOZ 
Nozzle radius 
DTHNOZ 
Azimuthal  angle  (in  degrees  measured  counterclockwise)  of  the
injector nozzle from the j = 1 plane.
VARIABLE   
TILTXY 
DESCRIPTION 
Rotation angle (in degrees) of the injector in the x-y plane, where 0.0 
points  towards  the  3  o’clock  position  (j = 1  line),  and  the  angle 
increases counterclockwise from there. 
TILTXZ 
Inclination angle (in degrees) of the injection in the x-z plane, where 
0.0 points straight down, x > 0.0 points in the positive x direction, 
and x < 0.0 points in the negative x direction. 
CONE 
Spray mean cone angle (in degrees) for hollow cone spray; spray
cone angle (in degrees) for solid cone spray. 
DCONE 
Injection liquid jet thickness in degrees. 
ANOZ 
Area of injector 
AMP0 
Initial amplitude of droplet oscillation at injector 
Remarks: 
1.  When IEVAP = 1, the keyword input file must be modified in a fashion similar to a 
chemistry problem.  This is illustrated in a portion of an example keyword file 
below.  That is, the following keywords need to be used, along with the inclusion 
of other chemistry-related files (i.e.  evap.inp and the corresponding thermody-
namics data file):   
*CHEMISTRY_MODEL 
*CHEMISTRY_COMPOSITION 
*CHEMISTRY_CONTROL_FULL 
*CESE_INITIAL_CHEMISTRY 
$ Setup stochastic particles 
$ 
*STOCHASTIC_SPRAY_PARTICLES 
$  injdist    ibrkup  icollide     ievap    ipulse    limprt    fuelid 
         3         1         0         1         0    100000         1 
$     rhop       tip pmass[Kg]    prtrte   str_inj   dur_inj 
    1000.0      300.      0.01     1.0e7       0.0      10.0 
$  the next card is needed for fireball position and max.  particle velocity: 
$    XORIG     YORIG     ZORIG       SMR   Velinj      Drnoz    Dthnoz 
     0.005     0.005    1.0e-5    5.0e-6    200.0     9.0e-5 
$   TILTXY    TILTXZ      CONE     DCONE     ANOZ       AMP0 
       0.0       0.0      15.0      15.0   2.5e-8        0.0 
$ 
*CHEMISTRY_MODEL 
$ model_id    jacsel    errlim
10         1       0.0 
  evap.inp 
 therm.dat 
  tran.dat 
$ 
*CHEMISTRY_COMPOSITION 
$  comp_id  model_id 
        11        10 
$  molefra   Species 
       1.0        O2 
      3.76        N2 
$ 
*CHEMISTRY_CONTROL_FULL 
$   sol_id    errlim 
         5 
$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ 
$ 
$ Set global initial conditions for fluid 
$ 
*CESE_INITIAL_CHEMISTRY 
$   sol_id   comp_id 
         5        11 
$INITIAL CONDITIONS  
$      uic       vic       wic       ric       pic       tic       hic    
       0.0       0.0       0.0       1.2   101325.     300.0       0.0
*STOCHASTIC_TBX_PARTICLES 
Purpose:    Specify  particle  and  other  model  details  for  stochastic  PDEs  that  model 
embedded  particles  in  TBX  explosives.    Note  that  the  components  listed  on  the 
corresponding *CHEMISTRY_COMPOSITION card are in terms of molar concentrations of 
the species (in units of moles/[length]3, where “[length]” is the user’s length unit). 
For further information on the theory of the TBX model that has been implemented, a 
document on this topic can be found at this URL: 
http://www.lstc.com/applications/cese_cfd/documentation 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
PCOMB 
NPRTCL  MXCNT 
PMASS 
SMR 
RHOP 
TICP 
T_IGNIT 
Type 
Default 
I 
0 
I 
I 
F 
F 
F 
F 
F 
none 
none 
none 
none 
none 
none 
none 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
INITDST 
AZIMTH 
ALTITD 
CPS/CVS 
HVAP 
EMISS 
BOLTZ 
Type 
Default 
I 
1 
Remarks 
F 
F 
F 
F 
F 
F 
none 
none 
none 
none 
none 
none 
1 
6 
1 
7 
8 
  Card 3 
1 
2 
3 
4 
5 
Variable 
XORIG 
YORIG 
ZORIG 
XVEL 
YVEL 
ZVEL 
FRADIUS 
Type 
F 
F 
F 
F 
F 
F 
F 
Default 
none 
none 
none 
0.0 
0.0 
0.0 
none
VARIABLE   
DESCRIPTION 
PCOMB 
Particle combustion model 
EQ.0: no burning 
EQ.1: K-model 
NPRTCL 
MXCNT 
Initial  total  number  of  parent  particles  (discrete  particles  for 
calculation) 
Maximum  allowed  number  of  parent  particles  (during  the
simulation) 
PMASS 
Total particle mass 
SMR 
Sort mean particle radius 
RHOP 
Particle density 
TICP 
Initial particle temperature 
T_IGNIT 
Particle ignition temperature 
INITDST 
Initial particle distribution 
EQ.1: spatially uniform 
EQ.2: Rosin-Rammler 
EQ.3: Chi-squared 
AZIMTH 
ALTITD 
Angle in degrees from 𝑥-axis in 𝑥-𝑦 plane of reference frame of TBX 
explosive (0 < AZMITH < 360) 
Angle in degrees from 𝑧-axis of reference frame of TBX explosive 
(0 < ALTITD < 180) 
CPS/CVS 
Heat coefficient 
HVAP 
EMISS 
Latent heat of vaporization 
Particle emissivity 
BOLTZ 
Boltzmann coefficient 
XORIG 
𝑥-coordinate of the origin of the initial reference frame of the TBX 
explosive
VARIABLE   
DESCRIPTION 
YORIG 
ZORIG 
XVEL 
YVEL 
ZVEL 
𝑦-coordinate of the origin of the initial reference frame of the TBX
explosive 
𝑧-coordinate of the origin of the initial reference frame of the TBX
explosive 
𝑥-component of the initial particle velocity the TBX explosive 
𝑦-component of the initial particle velocity the TBX explosive 
𝑧-component of the initial particle velocity the TBX explosive 
FRADIUS 
Radius of the explosive area. 
Remarks: 
1. 
If radiation heat transfer is being modeled, then EMISS and BOLTZ are required.
*LSO 
These cards provide a general data output mechanism, causing the creation of a sequence 
of LSDA files.  This facility is intended to allow several different time sequences of data to 
be output in the same simulation.  In addition, any number of domains (and any number of 
variables on those domains) may be specified within each time sequence.  The keyword 
cards in this section are defined in alphabetical order: 
*LSO_DOMAIN 
*LSO_ID_SET (not available in the single-precision version of LS-DYNA) 
*LSO_POINT_SET 
*LSO_TIME_SEQUENCE 
*LSO_VARIABLE_GROUP 
Note  that  only  the  mechanics  solver  is  available  in  the  single-precision  version  of  LS-
DYNA, and therefore, only LSO mechanics variables are available for output from single 
precision LS-DYNA.   These mechanics variables are listed by domain type in a separate 
document.  This document (LSO_VARIABLES.TXT) is created by running the command: 
LS-DYNA print_lso_doc.  Contrary to LSO_VARIABLES.TXT,   element quantities such as 
stress are not available for output from the mechanics solver to the “lso” database. 
An additional option “_TITLE” may be appended to all *LSO keywords.  If this option is 
used, then an 80 character string is read as a title from the first card of that keyword's 
input.  At present, LS-DYNA does not make use of the title.  Inclusion of titles gives greater 
clarity to input decks.
*LSO_DOMAIN 
Purpose: This command provides a way to specify variables on a subset of the domain for a 
given solver.  This domain can be a subset of the mesh used by that solver, a set of output 
points created with *LSO_POINT_SET, or a set of objects created with *LSO_ID_SET.  The 
frequency and duration of the output for any given domain is determined by each *LSO_-
TIME_SEQUENCE card that references this *LSO_DOMAIN card. Note that for the single-
precision version of LS-DYNA, the only allowed value of SOLVER_NAME = MECH. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
DOMAIN_TYPE 
A 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
SOLVER_NAME 
A 
Special  Domains  Card.  Card  3  when  DOMAIN_TYPE  is  one  of  ROGO,  CIRCUIT, 
THIST_POINT or TRACER_POINT. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OUTID 
REFID 
REDUCT 
Type 
I 
I 
I 
Default 
none 
none 
none
Miscellaneous Domain Card. Card 3 when DOMAIN_TYPE is one of NODE, PART, SEG-
MENT,  SURFACE_NODE,  SURFACE_ELEMENT,  VOLUME_ELEMENT,  SURFACE_-
PART, VOLUME_PART. 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
OUTID 
REFID  OVERRIDE REDUCT 
Type 
I 
Default 
none 
I 
0 
I 
0 
I 
none 
Variable Name Card. Provide as many cards as necessary.  This input ends at the next 
keyword (“*”) card 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
VARIABLE_NAME 
A 
  VARIABLE   
DESCRIPTION
DOMAIN_TYPE 
The type of domain for which LSO output may be generated.
SOLVER_NAME 
Selects the solver from which data is output on this domain.
Accepted  entries  so  far  are  “MECH”,  “EM”,  “CESE”,  and
“ICFD”. 
OUTID 
REFID 
LSO  domain  ID  associated  with  this  domain,  and  used  by
*LSO_TIME_SEQUENCE cards. 
Support set ID.  This can be a set defined by a *SET card, a
*LSO_ID_SET,  card,  or  a  *LSO_POINT_SET  card.    Unless 
OVERRIDE is specified, this set must be of the same type as
DOMAIN_TYPE. 
OVERRIDE 
If non-zero, then REFID is interpreted as: 
EQ.1: a PART set for SOLVER_NAME 
EQ.2: a PART set of volume parts created with a *LSO_-
ID_SET  card  (volume  parts  are  defined  with
*MESH_VOLUME cards).
EM 
ICFD 
CESE 
magneticField_point 
electricField_point 
vecpotField_point 
currentDensity2_point 
ScalarPotential_point 
velocity_point 
velocity_point 
pressure_point 
pressure_point 
temperature_point 
temperature_point 
density_point 
density_point 
lset_point 
Table 8-1.  Selected LSO Varriables 
  VARIABLE   
DESCRIPTION
REDUCT 
EQ.3: a PART set of surface parts created with a *LSO_ID_-
SET card (surface parts are defined with *MESH_-
SURFACE_ELEMENT cards). 
EQ.4: a set of segment sets created with a *LSO_ID_SET 
card. 
A function that operates on the entire domain and returns a
single  value  for  scalar  variables,  three  values  for  vector
variables,  or  6  values  for  symmetric  tensor  variables.    For
REDUCT=“range”, the number of returned values doubles.
The following are the supported functions: 
EQ.BLANK: 
no reduction (default) 
EQ.“none”: 
Same as above 
EQ.“avg”: 
the average by component 
EQ.“average”:  Same as above 
EQ.“min”: 
the minimum by component 
EQ.“minimum”:  Same as above 
EQ.“max”: 
the maximum by component 
EQ.“maximum”:  Same as above 
EQ.“sum”: 
the sum by component 
EQ.“range”: 
the minimum by component followed by
*LSO 
DESCRIPTION
the maximum by component 
VARIABLE_NAME 
Either  the  name  of  a  single  output  variable  or  a  variable
group.  See remarks. 
Remarks: 
1.  Supported choices for VARIABLE_NAME are listed by DOMAIN_TYPE for each 
SOLVER_NAME in a separate document.  This document (LSO_VARIABLES.TXT) 
is created by running the command: LS-DYNA print_lso_doc.  The following table 
shows    a  sample  of  the  point  output  variables  available  when  DOMAIN_-
TYPE = THIST_POINT:
*LSO_ID_SET 
Purpose:  Provides a way to create a set of existing sets (segment sets), or to define a set 
that is not available with other set-related keyword cards.  These are then used in other 
*LSO cards to specify LSO output.  This card is not available in the single precision version 
of LS-DYNA. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SETID 
TYPE 
SOLVER 
Type 
I 
A 
A 
Default 
none 
none  MECH 
Referenced IDs. Provide as many cards as necessary.  This input ends at the next keyword 
(“*”) card 
Card 
1 
Variable 
ID1 
2 
ID2 
3 
ID3 
4 
ID4 
5 
ID5 
6 
ID6 
7 
ID7 
8 
ID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
SETID 
Identifier for this ID set.
DESCRIPTION 
TYPE 
The kind of IDs in this set: 
*LSO 
EQ.’SEG_SETS’: 
Each  ID  is  a  segment  set  connected  with 
SOLVER. 
EQ.’CIRCUIT’: 
Each ID is a circuit ID (from *EM cards) 
EQ.’SURF_PARTS’:  Each  ID  is  a  surface  part  number   
EQ.’VOL_PARTS’:  Each  ID  is  a  volume  part  number   
EQ.’SURF_ELES’:  Each  ID  is  a  surface  element  number   
SOLVER 
Name of the solver (MECH, ICFD, CESE, EM, …) 
ID1, … 
IDs of the TYPE kind.
*LSO_POINT_SET 
Purpose:  Define a list of points used to sample variables in time.  Of the different sampling 
methods, the most common one is to specify points for time history output. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
SETID 
USE 
Type 
I 
Default 
none 
Remarks 
I 
1 
1 
Point Cards. Provide as many cards as necessary.  This input ends at the next keyword 
(“*”) card 
4 
5 
6 
7 
8 
Card 
Variable 
Type 
1 
X 
F 
2 
Y 
F 
3 
Z 
F 
Default 
none 
none 
none 
  VARIABLE   
DESCRIPTION 
SETID 
Identifier for this point set.  Used by *LSO_DOMAIN 
USE 
Points in this set are used as: 
EQ.1: Fixed time history points (default) 
EQ.2: Positions of tracer particles 
X, Y, Z 
Coordinates of a point.  As many points as desired can be specified.
*LSO 
1.  For USE = 1, with the ICFD and CESE solvers, the fixed points have to remain 
inside the fluid  mesh  or a zero result is returned, while for the EM solver, the 
points can be defined inside the conductors or in the air.  In the latter case, the 
fields will be computed using a Biot-Savart type integration. For USE = 2, a mass-
less tracer particle is tracked for the ICFD and CESE solvers using their local veloc-
ity field to integrate the position of each particle in time.
*LSO_TIME_SEQUENCE 
Purpose:  This command provides users with maximum flexibility in specifying exactly 
what they want to have appear in the output LSO binary database.  Each instance of the 
*LSO_TIME_SEQUENCE command creates  a new time sequence  with an independent 
output frequency and duration.  Furthermore, while the default domain for each output 
variable will be the entire mesh on which that variable is defined, at all selected snapshot 
times, the *LSO_DOMAIN keyword commands can be used to specify that output will only 
occur on a portion of SOLVER_NAME’s mesh, and for a limited time interval, or that it will 
occur at a set of points , or over a set of object IDs .  Note that for the single-precision version of LS-DYNA, the only allowed value of 
SOLVER_NAME = MECH. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
  Card 2 
Variable 
1 
DT 
Type 
F 
Default 
0.0 
Remarks 
1 
SOLVER_NAME 
A 
2 
3 
4 
5 
6 
7 
8 
LCDT 
LCOPT 
NPLTC 
TBEG 
TEND 
I 
0 
1 
I 
1 
1 
I 
0 
1 
F 
F 
0.0 
0.0
Domain IDs.  Provide as many cards as necessary.  This input ends at the next keyword 
(“*”) card, or when a global variable name card appears 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
DOMID1  DOMID2  DOMID3  DOMID4  DOMID5  DOMID6  DOMID7  DOMID8 
Type 
I 
I 
I 
I 
I 
I 
I 
I 
Default 
none 
none 
none 
none 
none 
none 
none 
none 
Global variable names.  Provide as many cards as necessary.  This input ends at the next 
keyword (“*”) card 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
GLOBAL_VAR 
A 
  VARIABLE   
DESCRIPTION
SOLVER_
NAME 
Selects the solver from which data is output in this time sequence.
Accepted entries so far are ‘MECH’, ‘EM’, ‘CESE’ and ‘ICFD’ 
DT 
LCDT 
Time interval between outputs. 
Optional  load  curve  ID  specifying  the  time  interval  between 
dumps. 
LCOPT 
Flag to govern behavior of plot frequency load curve: 
EQ.1: At the time each plot is generated, the load curve value
is added to the current time to determine the next plot
time (this is the default behavior). 
EQ.2: At the time each plot is generated, the next plot time T is
computed  so  that  T = the  current  time  plus  the  load 
curve value at the time T. 
EQ.3: A plot is generated for each ordinate point in the load
curve definition.  The actual value of the load curve is
ignored.
VARIABLE   
DESCRIPTION
NPLTC 
DT = ENDTIM/NPLTC overrides DT specified in the first field.
TBEG 
TEND 
The problem time at which to begin writing output to this time
sequence 
The problem time at which to terminate writing output to this
time sequence 
DOMID1, … 
Output set ID defining the domain over which variable output is
to be performed in this time sequence.  Each DOMID refers to the 
domain identifier in an *LSO_DOMAIN keyword card. 
The name of a global output variable computed by SOLVER_-
NAME.  This variable must have a single value (scalar, vector, or
tensor), and therefore does not depend upon any DOMID.  Any 
number  of  such  variables  may  be  specified  with  a  given  time
sequence.  These variables are listed as having “global” domain
for  SOLVER_NAME  in  a  separate  document.    This  document 
(LSO_VARIABLES.TXT) is created by running the command: LS-
DYNA print_lso_doc. 
GLOBAL_VAR 
Remarks: 
1. 
If LCDT is nonzero, then it is used and DT and NPLTC are ignored.  If LCDT is 
zero and NPLTC is non-zero, then NPLTC determines the snapshot time incre-
ment.  If LCDT and NPLTC are both zero, then the minimum non-zero time in-
crement specified by DT is used to determine the snapshot times.
*LSO 
Purpose:  To provide a means of defining a shorthand name for a group of variables.  That 
is, wherever the given group name is used, it is replaced by the list of variables given in 
this command.  Note that for the single-precision version of LS-DYNA, the only allowed 
value of SOLVER_NAME = MECH. 
  Card 1 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
SOLVER_NAME 
A 
  Card 2 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
DOMAIN_TYPE 
A 
  Card 3 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
GROUP_NAME 
A 
List Of Variables In Group.  Provide as many cards as necessary.  This input ends at the 
next keyword (“*”) card 
  Card 4 
1 
2 
3 
4 
5 
6 
7 
8 
Variable 
Type 
VAR_NAME 
A 
  VARIABLE   
DESCRIPTION
SOLVER_NAME 
Selects the solver for which data is output in a time sequence.
DOMAIN_TYPE 
*LSO_VARIABLE_GROUP 
DESCRIPTION
Name  of  the  type  of  domain  on  which  each  VAR_NAME  is 
defined. 
GROUP_NAME 
Name of (or alias for) the group of names given by the listed
VAR_NAMEs 
VAR_NAME 
The name of an output variable computed by SOLVER_NAME
Remarks: 
1.  Valid VAR_NAMEs depend both upon the SOLVER_NAME and the DOMAIN_-
TYPE.  These variables are listed by DOMAIN_TYPE for each SOLVER_NAME in 
a separate document.  This document (LSO_VARIABLES.TXT) is created by run-
ning the command: LS-DYNA print_lso_doc.


Introduction 
This document presents  some  LS-DYNA examples providing  a basic  guide in  different 
disciplines like: 
•  Structural static (stress analysis, buckling analysis and modal analysis) 
•  Structural dynamic (vibrations and impact) 
•  Thermal analysis (heat transfer via conduction, convection and radiation) 
This guide is mainly addressed to first-time users.  The input files are always present for 
each  problem,  using  the  KEYWORD  input  format.    For  sake  of  briefness,  in  most 
problems the full node and element definitions (also, some load segments) are omitted. 
Several  of  the  problems  present  a  closed-form  solution,  while  others  (the  majority)  a 
reference solution obtained by using an arbitrary refined mesh (NAFEMS Benchmarks).  
In these cases, the obtained value vs. the reference solution value is reported.  Most of the 
problems are implicit ones.  Problem-specific keywords are listed under the title of each 
problem. 
This guide refers to LS-DYNA v.971, but most of the problems also run on the 970, 960 
and 950 versions.  All problems have been tested using a double precision executable.
Benchmark References 
Example 1.  Skew Plate with Normal Pressure (thin shell mesh) 
The  Standard  NAFEMS  Benchmarks,  NAFEMS  Report  TNSB,  Rev.  3,  October,  1990, 
Test LE6. 
Example 2.  Skew Plate with Normal Pressure (thick shell mesh) 
The  Standard  NAFEMS  Benchmarks,  NAFEMS  Report  TNSB,  Rev.  3,  October,  1990, 
Test LE6. 
Example 3.  Elliptical Thick Plate under Normal Pressure (coarse mesh) 
Davies,  G.A.O.,  Fenner,  R.T.,  and  Lewis,  R.W.,  NAFEMS  Background  to  Benchmarks, 
June, 1992, Test LE10. 
Example 4.  Elliptical Thick Plate under Normal Pressure (fine mesh) 
Davies,  G.A.O.,  Fenner,  R.T.,  and  Lewis,  R.W.,  NAFEMS  Background  to  Benchmarks, 
June, 1992, Test LE10. 
Example 5.  Snap-Back under Displacement Control 
NAFEMS Non-Linear Benchmarks, NAFEMS Report NNB, Rev. 1, October, 1989, Test 
NL4. 
Example 6.  Straight Cantilever Beam with Axial End Point Load 
NAFEMS Non-Linear Benchmarks, NAFEMS Report NNB, Rev. 1, October, 1989, Test 
NL6. 
Example 7.  Lee's Frame Buckling Problem 
NAFEMS Non-Linear Benchmarks, NAFEMS Report NNB, Rev. 1, October, 1989, Test 
NL7. 
Example 8.  Pin-Ended Double Cross: In-Plane Vibration 
The  Standard  NAFEMS  Benchmarks,  NAFEMS  Report  TNSB,  Rev.  3,  October,  1990, 
Test FV2. 
Example 9.  Simply Supported Thin Annular Plate (coarse mesh) 
Abbassian,  F.,  Dawswell,  D.J.,  and  Knowles,  N.C.,  NAFEMS  Selected  Benchmarks  for 
Natural Frequency Analysis, November, 1987, Test 14. 
Example 10.  Simply Supported Thin Annular Plate (fine mesh) 
Abbassian,  F.,  Dawswell,  D.J.,  and  Knowles,  N.C.,  NAFEMS  Selected  Benchmarks  for 
Natural Frequency Analysis, November, 1987, Test 14. 
Example 11.  Transient Response to a Constant Force
Example 12.  Simply Supported Square Plate: Out-of Plane Vibration (solid mesh) 
Abbassian,  F.,  Dawswell,  D.J.,  and  Knowles,  N.C.,  NAFEMS  Free  Vibration 
Benchmarks, October, 2001, Test FV52. 
Example 13.  Simply Supported Square Plate: Out-of-Plane Vibration (thick shell mesh) 
Abbassian,  F.,  Dawswell,  D.J.,  and  Knowles,  N.C.,  NAFEMS  Free  Vibration 
Benchmarks, October, 2001, Test FV52. 
Example 14.  Simply Supported Square Plate: Transient Forced Vibration (solid mesh) 
Maguire,  J.,  Dawswell,  D.J.,  and  Gould,  L.,NAFEMS  Selected  Benchmarks  for  Forced 
Vibration, February, 1989, Test 21T. 
Example  15.    Simply  Supported  Square  Plate:  Transient  Forced  Vibration  (thick  shell 
mesh) 
Maguire, J., Dawswell,  D.J., and  Gould,  L., NAFEMS Selected  Benchmarks for Forced 
Vibration, February, 1989, Test 21T. 
Example 16.  Transient Response of a Cylindrical Disk Impacting a Deformable Surface 
Thomson,  W.T.,  Vibration  Theory  and  Applications,  2nd  Printing,  Prentice-Hall,  Inc., 
Englewood Cliffs, New Jersey, 1965, pg. 110, ex. 4.6-1. 
Example 17.  Natural Frequency of a Linear Spring-Mass System 
Timoshenko, S.P., and Young, D.H., Vibration Problems in Engineering, 3rd Edition, D. 
Van Nostrand Co., Inc., New York, New York, 1955, pg.1. 
Example 18.  Natural Frequency of a Nonlinear Spring-Mass System 
Timoshenko, S.P., and Young, D.H., Vibration Problems in Engineering, 3rd Edition, D. 
Van Nostrand Co., Inc., New York, New York, 1955, pg. 141. 
Example 19.  Buckling of a Thin Walled Cylinder Under Compression 
Timoshenko,  S.P.,  and  Gere,  J.M.,  Theory  of  Elastic  Stability,  McGraw-Hill  Book  Co., 
Inc., New York, New York, 1961, pg. 457. 
Example 20.  Membrane with a Hot Spot 
Davies,  G.A.O.,  Fenner,  R.T.,  and  Lewis,  R.W.,  NAFEMS  Background  to  Benchmarks, 
June, 1992, Test T1. 
Example 21.  1D Transient Heat Transfer with Radiation 
Davies,  G.A.O.,  Fenner,  R.T.,  and  Lewis,  R.W.,  NAFEMS  Background  to  Benchmarks, 
June, 1992, Test T2. 
Example 22.  1D Transient Heat Transfer in a Bar
Example 23.  2D Heat Transfer with Convection 
Davies,  G.A.O.,  Fenner,  R.T.,  and  Lewis,  R.W.,  NAFEMS  Background  to  Benchmarks, 
June, 1992, Test T4. 
Example 24.  3D Thermal Load 
Davies,  G.A.O.,  Fenner,  R.T.,  and  Lewis,  R.W.,  NAFEMS  Background  to  Benchmarks, 
June, 1992, Test LE11. 
Example 25.  Cooling of a Billet via Radiation 
Siegal, R., and Howell, J.R., Thermal Radiation Heat Transfer, 3rd Edition, Hemisphere 
Publishing Corporation, 1981, pg. 229, problem 21. 
Example 26.  Pipe Whip 
Lerencz,  R.M.,  Element-by-Element  Preconditioning  Techniques  for  Large-Scale, 
Vectorized Finite Element Analysis in Nonlinear Solid and Structural Mechanics, Ph.D. 
Thesis,  Department  of  Mechanical  Engineering,  Stanford  University,  Palo  Alto, 
California, March, 1989, pg. 142, pipe whip. 
Example 27.  Aluminum Bar Impacting a Rigid Wall 
Lerencz,  R.M.,  Element-by-Element  Preconditioning  Techniques  for  Large-Scale, 
Vectorized Finite Element Analysis in Nonlinear Solid and Structural Mechanics, Ph.D.
1. 
Skew Plate with Normal Pressure (thin shell mesh) 
Keywords: 
*CONTROL_IMPLICIT_GENERAL 
*CONTROL_IMPLICIT_SOLUTION 
Description: 
A skew plate of equal side lengths L and thickness t is subjected to a normal pressure P 
on the top face (Figure 1.1).  The plate is meshed with thin shell elements with a 4 x 4 
ZU = .    Determine  the 
density.    The  plate  is  simply  supported  on  four  side  faces, 
maximum principal stress at plate center point E on the bottom surface. 
Figure 1.1 – Sketch representing the structure. 
Analysis Summary: 
Dim.  Type 
Load  Material  Geometry  Contact 
Solver 
Solution 
Method 
3D 
Static  Pressure  Linear 
Linear 
- 
Implicit 
1-Linear 
Units:
Dimensional Data: 
=
1.0
, 
=
0.01
Material Data: 
Mass Density 
Young's Modulus 
Poisson's Ratio 
ρ=
=
ν =
11
×
7.80 10
×
2.07 10
0.3
/kg m
Pa
Load: 
Pressure 
Element Types: 
=
×
7.0 10
Pa
Belytschko-Tsay shell (elform=2) 
S/R Hughes-Liu shell (elform=6) 
Fully integrated shell (elform=16) 
Material Models: 
*MAT_001 or *MAT_ELASTIC 
Results Comparison: 
LS-DYNA maximum principal stress at plate center Point E (Node 13) on bottom surface 
ZU ,  are  compared  with  Standard  NAFEMS  Benchmarks,  Test 
plus  its  Z-displacement,
LE6. 
Reference Condition - Point E (Node 13) 
Max Principal 
Stress (Pa) 
ZU (m) 
NAFEMS Benchmark Test LE6 
0.802 10×
- 
Belytschko-Tsay shell (elform=2) 
0.781 10×
1.616 10−
×
−
S/R Hughes-Liu shell (elform=6) 
0.715 10×
1.507 10−
×
−
Fully integrated shell (elform=16) 
0.696 10×
1.404 10−
×
−
These nodal displacement results were generated by *DATABASE_NODOUT keyword 
while the maximum principal stress results were generated by *DATABASE_ ELOUT. 
LS-DYNA stress and strain output corresponds to integration point locations.  Stress at a 
node  is  an  artifact  of  the  post-processor  and  represents  an  average  of  the  surrounding 
integration  point  stresses  (the  value  will  likely  be  different  with  different  post-
processors). 
Lobatto  integration  (intgrd=1  -  *CONTROL_SHELL)  was  employed  since  it  has  an 
advantage in that the inner and outer integration points are on the shell surfaces.  Gauss 
integration  is  the  default  through  thickness  integration  rule  (the  default  number  of 
through thickness integration points is nip=2 - *SECTION_SHELL) in LS-DYNA, where 
1-10  integration  points  may  be  specified,  whereas,  with  Lobatto  integration,  3-10 
integration  points  may  be  specified  (for  2  point  integration,  the  Lobatto  rule  is  very 
inaccurate). 
For  this  coarse  meshing,  the  one-point  quadrature  (low  order)  Belytschko-Tsay  shell 
(elform=2) provides a good stress comparison (Figure 1.2). 
The  higher  order,  selectively  reduced  integration  Hughes-Liu  shell  (elform=6)  and  the 
fully  integrated  Belytschko-Tsay  shell  (elform=16),  which  uses  a  2x2  in-plane 
quadrature, provide comparatively stiffer results (Figure 1.3 and 1.4), probably due to the 
coarse meshing.
Figure 1.3 – Element formulation 6 (S/R Hughes-Liu).
*TITLE 
Skew Plate with Normal Pressure (thin shell mesh) 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form 
         1       0.0         2         1         2 
*CONTROL_IMPLICIT_SOLUTION 
$#  nsolvr    ilimit    maxref     dctol     ectol     rctol     lstol    abstol 
         1        11        15  0.001000  0.010000       0.0  0.900000  1.000000 
$#   dnorm    diverg     istif   nlprint 
         2         1         1         2 
$#  arcctl    arcdir    arclen    arcmth    arcdmp 
         0         1       0.0         1         2 
*CONTROL_SHELL 
$#  wrpang     esort     irnxx    istupd    theory       bwc     miter      proj 
  20.00000         0         0         0         2         2         1 
$# rotascl    intgrd    lamsht    cstyp6    tshell    nfail1    nfail4 
       0.0         1 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
  1.000000         0       0.0       0.0       0.0 
*DATABASE_ELOUT 
$# .....dt 
   1.0E-01 
*DATABASE_BINARY_D3PLOT 
$# dt/cycl 
  0.100000 
*DATABASE_HISTORY_SHELL 
$#    eid1      eid2      eid3      eid4       ei5      eid6      eid7      eid8 
         6         7        10        11 
*DEFINE_CURVE 
$#    lcid      sdir       sfa       sfo      offa      offo     dattyp 
         1         0       0.0       0.0       0.0       0.0 
$#                a1                  o1 
                 0.0                 0.0 
          1.00000000         700.0000000 
*ELEMENT_SHELL 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       1       6       7       2 
      16       1      19      24      25      20 
*NODE 
$#   nid               x               y               z      tc      rc 
       1             0.0             0.0             0.0       3 
      25      1.86602540      0.50000000             0.0       3 
*PART 
$# title                                                                         
material type # 1  (Elastic)                                                     
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1 
*SECTION_SHELL 
$#   secid    elform      shrf       nip     propt   qr/irid     icomp     setyp 
         1         2       0.0         5         0       0.0 
$         1         6       0.0         5         0       0.0 
$         1        16       0.0         5         0       0.0 
$#      t1        t2        t3        t4      nloc     marea 
  0.010000  0.010000  0.010000  0.010000         0       0.0 
*MAT_ELASTIC 
$#     mid        ro         e        pr        da        db  not used 
         1  7800.0002.1000e+11  0.300000       0.0       0.0       0.0 
*LOAD_SEGMENT 
$#    lcid        sf        at        n1        n2        n3        n4 
         1  1.000000       0.0         1         6         7         2 
         1  1.000000       0.0         2         7         8         3 
         1  1.000000       0.0         3         8         9         4 
         1  1.000000       0.0         4         9        10         5
1  1.000000       0.0         7        12        13         8 
         1  1.000000       0.0         8        13        14         9 
         1  1.000000       0.0         9        14        15        10 
         1  1.000000       0.0        11        16        17        12 
         1  1.000000       0.0        12        17        18        13 
         1  1.000000       0.0        13        18        19        14 
         1  1.000000       0.0        14        19        20        15 
         1  1.000000       0.0        16        21        22        17 
         1  1.000000       0.0        17        22        23        18 
         1  1.000000       0.0        18        23        24        19 
         1  1.000000       0.0        19        24        25        20 
*END
2. 
Skew Plate with Normal Pressure (thick shell mesh) 
Keywords: 
*CONTROL_IMPLICIT_GENERAL 
*CONTROL_IMPLICIT_SOLUTION 
Description: 
A skew plate of equal side lengths L and thickness t is subjected to a normal pressure P 
on the top face (Figure 2.1).  The plate is meshed with thick shell elements with a 4 x 4 
ZU = .  
density.  The plate is simply supported on four side faces of the bottom surface, 
Determine the maximum principal stress at plate center point E on the bottom surface. 
Figure 2.1 – Sketch representing the structure. 
Analysis Summary: 
Dim.  Type 
Load  Material  Geometry  Contact 
Solver 
Solution 
Method 
3D 
Static  Pressure  Linear 
Linear 
- 
Implicit 
1-Linear 
Units:
Dimensional Data: 
=
1.0
, 
=
0.01
Material Data: 
Mass Density 
Young's Modulus 
Poisson's Ratio 
ρ=
=
ν =
11
×
7.80 10
×
2.07 10
0.3
/kg m
Pa
Load: 
Pressure 
Element Types: 
=
×
7.0 10
Pa
S/R 2x2 IPI thick shell (elform=2) 
Assumed strain 2x2 IPI thick shell (elform=3) 
Assumed strain RI thick shell (elform=5) 
Material Models: 
*MAT_001 or *MAT_ELASTIC 
Results Comparison: 
LS-DYNA  maximum  principal  stress  at  plate  center  Point  E  (Node  113)  on  bottom 
ZU , are compared with Standard NAFEMS Benchmarks, 
surface plus its Z-displacement,
Test LE6. 
Reference Condition - Point E (Node113) 
Max Principal 
Stress (Pa) 
ZU (m) 
NAFEMS Benchmark Test LE6 
0.802 10×
- 
S/R 2x2 IPI thick shell (elform=2) 
0.709 10×
1.496 10−
×
−
Assumed strain 2x2 IPI thick shell 
(elform=3) 
0.021 10×
est. 
0.084 10−
×
−
Assumed strain RI thick shell (elform=5) 
0.211 10×
0.849 10−
×
−
These nodal displacement results were generated by *DATABASE_NODOUT keyword 
while 
results  were  generated  by 
*DATABASE_ELOUT. 
the  maximum  principal 
(nodal) 
stress 
At least two elements through the thickness are usually recommended to capture bending 
response  for assumed strain 2x2  IPI thick  shell (elform=3)  and  assumed  strain RI thick 
shell (elform=5) formulations. 
LS-DYNA stress and strain output corresponds to integration point locations.  Stress at a 
node  is  an  artifact  of  the  post-processor  and  represents  an  average  of  the  surrounding 
integration  point  stresses  (the  value  will  likely  be  different  with  different  post-
processors). 
Lobatto  integration  (intgrd=1  -  *CONTROL_SHELL)  was  employed  since  it  has  an 
advantage in that the inner and outer integration points are on the shell surfaces.  Gauss 
integration  is  the  default  through  thickness  integration  rule  (the  default  number  of 
through  thickness  integration  points  is  nip=2  -  *SECTION_TSHELL)  in  LS-DYNA, 
where 1-10 integration points may be specified, whereas, with Lobatto integration, 3-10 
integration  points  may  be  specified  (for  2  point  integration,  the  Lobatto  rule  is  very 
inaccurate). 
Only  the  higher  order  selectively  reduced  2x2  IPI  thick  shell  (elform=2)  provides  a 
reasonable  stress  comparison  (Figure  2.2).    As  with  other  higher  order  options,  this 
formulation  provides  a  comparatively  stiff  result,  again  probably  due  to  the  coarse 
meshing. 
The  higher  order  assumed  strain  2x2  IPI  thick  shell  (elform=3)  and  assumed  strain  RI 
thick shell (elform=5) formulations do  not  provide  acceptable  solutions (Figure 2.3 and 
2.4)  since  at  least  two  elements  through  the  thickness  are  usually  recommended  to
Figure 2.2 – Element formulation 2 (S/R 2x2 IPI).
Figure 2.4 - Element formulation 5 (assumed strain RI). 
Input Deck: 
*KEYWORD 
*TITLE 
Skew Plate with Normal Pressure (thick shell) 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form 
         1       0.0         2         1         2 
*CONTROL_IMPLICIT_SOLUTION 
$#  nsolvr    ilimit    maxref     dctol     ectol     rctol     lstol    abstol 
         1        11        15  0.001000  0.010000       0.0  0.900000  1.000000 
$#   dnorm    diverg     istif   nlprint 
         2         1         1         2 
$#  arcctl    arcdir    arclen    arcmth    arcdmp 
         0         1       0.0         1         2 
*CONTROL_SHELL 
$#  wrpang     esort     irnxx    istupd    theory       bwc     miter      proj 
  20.00000         0         0         0         2         2         1 
$# rotascl    intgrd    lamsht    cstyp6    tshell    nfail1    nfail4 
       0.0         1 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
  1.000000         0       0.0       0.0       0.0 
*DATABASE_ELOUT 
$# dt/cycl 
   1.0E-01 
*DATABASE_BINARY_D3PLOT 
$# dt/cycl 
  0.100000 
*DATABASE_HISTORY_TSHELL 
$#    eid1      eid2      eid3      eid4       ei5      eid6      eid7      eid8 
         6         7        10        11
$#    lcid      sdir       sfa       sfo      offa      offo     dattyp 
         1         0       0.0       0.0       0.0       0.0 
$#                a1                  o1 
                 0.0                 0.0 
          1.00000000         700.0000000 
*ELEMENT_TSHELL 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       1       6       7       2     101     106     107     102 
      16       1      19      24      25      20     119     124     125     120 
*NODE 
$#   nid               x               y               z      tc      rc 
       1             0.0             0.0             0.0       3 
     125      1.86602540      0.50000000           0.010 
*PART 
$# title                                                                         
material type # 1  (Elastic)                                                     
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1 
*SECTION_TSHELL 
$#   secid    elform      shrf       nip     propt   qr/irid     icomp    tshear 
         1         2       0.0         5         0       0.0 
$         1         3       0.0         5         0       0.0 
$         1         5       0.0         5         0       0.0 
*MAT_ELASTIC 
$#     mid        ro         e        pr        da        db  not used 
         1  7800.0002.1000e+11  0.300000       0.0       0.0       0.0 
*LOAD_SEGMENT 
$#    lcid        sf        at        n1        n2        n3        n4 
         1  1.000000       0.0       101       106       107       102 
         1  1.000000       0.0       102       107       108       103 
         1  1.000000       0.0       103       108       109       104 
         1  1.000000       0.0       104       109       110       105 
         1  1.000000       0.0       106       111       112       107 
         1  1.000000       0.0       107       112       113       108 
         1  1.000000       0.0       108       113       114       109 
         1  1.000000       0.0       109       114       115       110 
         1  1.000000       0.0       111       116       117       112 
         1  1.000000       0.0       112       117       118       113 
         1  1.000000       0.0       113       118       119       114 
         1  1.000000       0.0       114       119       120       115 
         1  1.000000       0.0       116       121       122       117 
         1  1.000000       0.0       117       122       123       118 
         1  1.000000       0.0       118       123       124       119 
         1  1.000000       0.0       119       124       125       120 
*END
3.  Elliptical Thick Plate under Normal Pressure (coarse 
mesh) 
Keywords: 
*CONTROL_IMPLICIT_GENERAL 
*CONTROL_IMPLICIT_SOLUTION 
*CONTROL_IMPLICIT_SOLVER 
Description: 
An  elliptical  thick  plate  with  thickness  t  is  subjected  to  a  normal  pressure  P  on  its  top 
surface (Figure 3.1).  The plate is meshed with solid hexahedra element with a 4 x 6 x 4 
YU = ; face ABB′A′ has no X-
density.  Face CC′D′D has no Y-direction displacement, 
XU = ;  the  X  and  Y  displacements  of  face  BCC′B′  are  fixed, 
= ;  and  the  mid-plane  (face  BCC'B')  has  no  X-,  Y-,  and  Z-direction 
= .    Determine  the  direct  stress  along  Y-direction  at  point 
direction  displacement, 
U=
=
=
displacement, 
D.
Analysis Summary: 
Dim.  Type 
Load  Material  Geometry  Contact 
Solver 
Solution 
Method 
3D 
Static  Pressure  Linear 
Linear 
- 
Implicit 
1-Linear 
Units: 
kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) 
Dimensional Data: 
=
1.0
, 
=
2.0
, 
=
1.75
, 
=
1.25
, 
=
0.60
Material Data: 
Mass Density 
Young's Modulus 
Poisson's Ratio 
ρ=
=
ν =
11
×
7.80 10
×
2.07 10
0.3
/kg m
Pa
Load: 
Pressure 
Element Types: 
=
×
1.0 10
Pa
Constant stress solid (elform=1) 
Fully integrated S/R solid (elform=2) 
Fully integrated S/R solid - for poor aspect ratio (eff) - (elform=-1) 
8 point enhanced strain solid (elform=18) 
Material Models: 
*MAT_001 or *MAT_ELASTIC 
Results Comparison: 
LS-DYNA Y-direction stress at plate edge Point D (Node 29) on top surface plus its Z-
ZU , are compared with NAFEMS Background to Benchmarks, Test LE10.
Reference Condition - Point D (Node 29) 
Axial Stress       
σyy  (Pa) 
ZU (m) 
NAFEMS Benchmark Test LE10 
−
×
5.38 10
- 
Constant stress solid (elform=1) 
−
×
4.78 10
est 
1.022 10−
×
−
Fully integrated S/R solid (elform=2) 
−
×
4.13 10
0.802 10−
×
−
Fully integrated S/R solid (elform=-1) 
−
×
5.35 10
1.005 10−
×
−
8 point enhanced strain solid (elform=18) 
−
×
6.40 10
0.973 10−
×
−
Estimated/extrapolated result calculated from 
−
3.67 10 Pa
×
 centroid value. 
These nodal displacement results were generated by *DATABASE_NODOUT keyword 
while  the  axial  stress  (nodal)  results  were  generated  by  *DATABASE_ELOUT  (elout 
file)  and  *DATABASE_EXTENT_BINARY  (eloutdet  file  provides  detailed  element 
output at integration points and connectivity nodes) keyword entries. 
You  can  set  intout=stress  or  intout=  all  (*DATABASE_EXTENT_BINARY)  and  have 
stresses  output 
file  called  eloutdet 
integration  points 
(*DATABASE_ELOUT  governs  the  output  interval  and  *DATABASE_HISTORY_ 
SOLID  governs  which  elements  are  output).    Setting  nodout=stress  or  nodout=all  in 
*DATABASE_EXTENT_BINARY will write the extrapolated nodal stresses to eloutdet. 
for  all 
to  a 
the 
LS-DYNA stress and strain output corresponds to integration point locations.  Stress at a 
node  is  an  artifact  of  the  post-processor  and  represents  an  average  of  the  surrounding 
integration  point  stresses  (the  value  will  likely  be  different  with  different  post-
processors). 
For  this  coarse  mesh,  the  one-point  quadrature  (low  order)  constant  stress  solid 
(elform=1) element formulation (the LS-DYNA default) provides a fair stress comparison 
(Figure 3.2).  Refinement of the mesh should provide a better comparison. 
The  higher  order,  fully  integrated  selectively  reduced  solid  (elform=2),  provides  a 
comparatively stiff result (Figure 3.3), probably due to the coarse meshing. 
The  aspect  ratio  of  the  elements  varies  throughout  the  coarse  meshing.    An  available
choice) intended to address poor aspect ratios (elform=-1).  This formulation provides a 
good comparison for this coarse meshing (Figure 3.4). 
The  8  point  enhanced  strain  solid  (elform=18),  developed  for  linear  statics  only,  over 
predicts the stress (Figure 3.5); no explanation is currently available.
Figure 3.3 – Element formulation 2 (fully integrated S/R).
Figure 3.5 – Element formulation 18 (8 point enhanced strain). 
Input Deck: 
*KEYWORD 
*TITLE 
Elliptical Thick Plate under Normal Pressure (coarse mesh) 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form 
         1  0.100000         2         1         2 
*CONTROL_IMPLICIT_SOLUTION 
$#  nsolvr    ilimit    maxref     dctol     ectol      rctol    lstol    abstol 
         1        11        15  0.001000  0.010000   1.00e+10 0.900000  1.00e-10 
*CONTROL_IMPLICIT_SOLVER 
$#  lsolvr    lprint     negev     order      drcm    drcprm   autospc   autotol 
         4         2         2         0         1       0.0         1       0.0 
$#  lcpack 
         2 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
  1.000000         0       0.0       0.0       0.0 
*DATABASE_ELOUT 
$#      dt    binary      lcur     ioopt 
 1.0000E-9         0         0          
*DATABASE_BINARY_D3PLOT 
$# dt/cycl 
  1.000000 
*DATABASE_EXTENT_BINARY 
$#   neiph     neips    maxint    strflg    sigflg    epsflg     rtflg    engflg 
$#  cmpflg    ieverp    beamip     dcomp      shge     stssz    n3thdt   ialemat 
$# nintsld   pkp_sen      sclp     hydro     msscl     therm    intout    nodout 
         8                 1.0                                  stress    stress 
*DATABASE_HISTORY_SOLID
$#    lcid      sdir       sfa       sfo      offa      offo     dattyp 
         1         0       0.0       0.0       0.0       0.0 
$#                a1                  o1 
                 0.0                 0.0 
          1.00000000       1.0000000e+06 
*ELEMENT_SOLID 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       1      10      13       4       2      11      14       5 
      96       1     168     172     174     170     169     173     175     171 
*NODE 
$#   nid               x               y               z      tc      rc 
       1      2.00000000             0.0             0.0       2 
     175             0.0      2.75000000      0.60000002       4 
*PART 
$# title                                                                         
material type # 1  (Elastic)                                                     
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1 
*SECTION_SOLID 
$#   secid    elform       aet 
         1         1         1 
$         1         2         1 
$         1        -1         1 
$         1        18         1 
*MAT_ELASTIC 
$#     mid        ro         e        pr        da        db  not used 
         1  7800.0002.1000e+11  0.300000       0.0       0.0       0.0 
*LOAD_SEGMENT 
$#    lcid        sf        at        n1        n2        n3        n4 
         1  1.000000       0.0        29        35        37        31 
         1  1.000000       0.0        31        37        39        33 
         1  1.000000       0.0        35        41        43        37 
         1  1.000000       0.0        37        43        45        39 
         1  1.000000       0.0        33        39        69        65 
         1  1.000000       0.0        65        69        71        67 
         1  1.000000       0.0        39        45        73        69 
         1  1.000000       0.0        69        73        75        71 
         1  1.000000       0.0        67        71        99        95 
         1  1.000000       0.0        95        99       101        97 
         1  1.000000       0.0        71        75       103        99 
         1  1.000000       0.0        99       103       105       101 
         1  1.000000       0.0        41       125       127        43 
         1  1.000000       0.0        43       127       129        45 
         1  1.000000       0.0       125       131       133       127 
         1  1.000000       0.0       127       133       135       129 
         1  1.000000       0.0        45       129       149        73 
         1  1.000000       0.0        73       149       151        75 
         1  1.000000       0.0       129       135       153       149 
         1  1.000000       0.0       149       153       155       151 
         1  1.000000       0.0        75       151       169       103 
         1  1.000000       0.0       103       169       171       105 
         1  1.000000       0.0       151       155       173       169 
         1  1.000000       0.0       169       173       175       171 
*END 
Notes: 
1.  One  should  remember  that  the  constant  stress  solid  (elform=1),  the  fully  integrated 
S/R  solid  (elform=2),  and  the  fully  integrated  S/R  solid  (the  so-called  efficient 
formulation choice) intended to address poor aspect ratios (elform=-1) were originally
4.  Elliptic Thick Plate under Normal Pressure (fine mesh) 
Keywords: 
*CONTROL_IMPLICIT_GENERAL 
*CONTROL_IMPLICIT_SOLUTION 
*CONTROL_IMPLICIT_SOLVER 
Description: 
An  elliptical  thick  plate  with  thickness  t  is  subjected  to  a  normal  pressure  P  on  its  top 
surface (Figure 4.1).  The plate is meshed with solid hexahedra element with an 8 x 12 x 
YU = ; face ABB′A′ has no 
4 density.   Face CC′D′D has no Y-direction displacement, 
XU = ; the X and Y displacements of face BCC′B′ are fixed, 
= ;  and  the  mid-plane  (face  BCC'B')  has  no  X-,  Y-,  and  Z-direction 
= .    Determine  the  direct  stress  along  Y-direction  at  point 
X-direction displacement, 
U=
=
=
displacement, 
D.
Analysis Summary: 
Dim.  Type 
Load  Material  Geometry  Contact 
Solver 
Solution 
Method 
3D 
Static  Pressure  Linear 
Linear 
- 
Implicit 
1-Linear 
Units: 
kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) 
Dimensional Data: 
=
1.0
, 
=
2.0
, 
=
1.75
, 
=
1.25
, 
=
0.60
Material Data: 
Mass Density 
Young's Modulus 
Poisson's Ratio 
ρ=
=
ν =
11
×
7.80 10
×
2.07 10
0.3
/kg m
Pa
Load: 
Pressure 
Element Types: 
=
×
1.0 10
Pa
Constant stress solid (elform=1) 
Fully integrated S/R solid (elform=2) 
Fully integrated S/R solid (elform=-1) 
8 point enhanced strain solid (elform=18) 
Material Models: 
*MAT_001 or *MAT_ELASTIC 
Results Comparison: 
LS-DYNA Y-direction stress at plate edge Point D (Node 77) on top surface plus its Z-
ZU , are compared with NAFEMS Background to Benchmarks, Test LE10.
Reference Condition - Point D (Node 77) 
Axial Stress       
σyy  (Pa) 
ZU (m) 
NAFEMS Benchmark Test LE10 
−
×
5.38 10
- 
Constant stress solid (elform=1) 
−
×
5.30 10
est 
1.051 10−
×
−
Fully integrated S/R solid (elform=2) 
−
×
4.70 10
0.947 10−
×
−
Fully integrated S/R solid (elform=-1) 
−
×
4.76 10
0.991 10−
×
−
8 point enhanced strain solid (elform=18) 
−
×
6.28 10
0.982 10−
×
−
Estimated/extrapolated result calculated from 
−
4.07 10 Pa
×
 centroid value. 
These nodal displacement results were generated by *DATABASE_NODOUT keyword 
while  the  axial  stress  (nodal)  results  were  generated  by  *DATABASE_ELOUT  (elout 
file)  and  *DATABASE_EXTENT_BINARY  (eloutdet  file  provides  detailed  element 
output at integration points and connectivity nodes) keyword entries. 
You  can  set  intout=stress  or  intout=all  (*DATABASE_EXTENT_BINARY)  and  have 
stresses  output 
file  called  eloutdet 
integration  points 
(*DATABASE_ELOUT  governs  the  output  interval  and  *DATABASE_HISTORY_ 
SOLID  governs  which  elements  are  output).    Setting  nodout=stress  or  nodout=all  in 
*DATABASE_EXTENT_BINARY will write the extrapolated nodal stresses to eloutdet. 
for  all 
to  a 
the 
LS-DYNA stress and strain output corresponds to integration point locations.  Stress at a 
node  is  an  artifact  of  the  post-processor  and  represents  an  average  of  the  surrounding 
integration  point  stresses  (the  value  will  likely  be  different  with  different  post-
processors). 
For this fine mesh, the one-point quadrature (low order) constant stress solid (elform=1) 
element formulation (the LS-DYNA default) provides a better stress comparison (Figure 
4.2), when compared to the coarse mesh. 
The  higher  order,  fully  integrated  selectively  reduced  solid  (elform=2)  still  provides  a 
comparatively stiff result (Figure 4.3); however, much improved over the coarse mesh. 
Doubling the elements in the x-y plane (mesh refinement) appears to have minimized the
(the  so-called  efficient  formulation  choice)  intended  to  address  poor  aspect  ratios 
(elform=-1)  now  provides  a  very  similar  result  (Figure  4.4)  to  the  fully  integrated  S/R 
solid (elform=2). 
The  8  point  enhanced  strain  solid  (elform=18),  developed  for  linear  statics  only,  over 
predicts  the  stress  result  (Figure  4.5)  by  a  fair  amount  (even  with  the  change  in  mesh 
refinement); no explanation is presently available.
Figure 4.3 – Element formulation 2 (fully integrated S/R).
Figure 4.5 – Element formulation 18 (8 point enhanced strain). 
Input Deck: 
*KEYWORD 
*TITLE 
Thick Elliptic Plate under Normal Pressure (fine mesh) 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form 
         1  0.100000         2         0         2 
*CONTROL_IMPLICIT_SOLUTION 
$#  nsolvr    ilimit    maxref     dctol     ectol      rctol    lstol    abstol 
         1        11        15  0.001000  0.010000   1.00e+10 0.900000  1.00e-10 
*CONTROL_IMPLICIT_SOLVER 
$#  lsolvr    lprint     negev     order      drcm    drcprm   autospc   autotol 
         4         2         2         0         0       0.0         0       0.0 
$#  lcpack 
         2 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
  1.000000         0       0.0       0.0       0.0 
*DATABASE_ELOUT 
$#      dt    binary      lcur     ioopt 
 1.0000E-9         0         0          
*DATABASE_BINARY_D3PLOT 
$# dt/cycl 
  1.000000 
*DATABASE_EXTENT_BINARY 
$#   neiph     neips    maxint    strflg    sigflg    epsflg     rtflg    engflg 
$#  cmpflg    ieverp    beamip     dcomp      shge     stssz    n3thdt   ialemat 
$# nintsld   pkp_sen      sclp     hydro     msscl     therm    intout    nodout 
         8                 1.0                                  stress    stress 
*DATABASE_HISTORY_SOLID 
$#     id1       id2       id3       id4       id5       id6       id7       id8
1         0       0.0       0.0       0.0       0.0 
$#                a1                  o1 
                 0.0                 0.0 
          1.00000000       1.0000000e+06 
*ELEMENT_SOLID 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       1      16      19       4       2      17      20       5 
     384       1     574     582     584     576     575     583     585     577 
*NODE 
$#   nid               x               y               z      tc      rc 
       1      2.00000000             0.0             0.0       2 
     585             0.0      2.75000000      0.60000002       4 
*PART 
$# title                                                                         
material type # 1  (Elastic)                                                     
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1 
*SECTION_SOLID 
$#   secid    elform       aet 
         1         1         1 
$         1         2         1 
$         1        -1         1 
$         1        18         1 
*MAT_ELASTIC 
$#     mid        ro         e        pr        da        db  not used 
         1  7800.000 2.100e+11  0.300000       0.0       0.0       0.0 
*LOAD_SEGMENT 
$#    lcid        sf        at        n1        n2        n3        n4 
         1  1.000000       0.0        77        87        89        79 
         1  1.000000       0.0        79        89        91        81 
         1  1.000000       0.0       575       583       585       577 
         1  1.000000       0.0       575       583       585       577 
*END 
Notes: 
1.  One  should  remember  that  the  constant  stress  solid  (elform=1),  the  fully  integrated 
S/R  solid  (elform=2),  and  the  fully  integrated  S/R  solid  (the  so-called  efficient 
formulation choice) intended to address poor aspect ratios (elform=-1) were originally
5. 
Snap-Back under Displacement Control 
Keywords: 
*CONTROL_IMPLICIT_AUTO 
*CONTROL_IMPLICIT_GENERAL 
*CONTROL_IMPLICIT_SOLUTION 
Description: 
In this problem the implicit arc length method is used in order to solve the snap-back of 
the system.  With traditional Newton-based methods it is not possible to fully solve this 
problem, due to the null tangent stiffness matrix at a certain point of the analysis. 
Three DOF are present. 
A  sketch  representing  the  structure  is  shown  below  (Figure  5.1)  along  with  a  finite 
element representation (Figure 5.2).
Figure 5.2 – The finite element representation of the problem.  Four beams are 
used; the springs are modeled with discrete formulation, the truss is modeled with 
truss formulation.  To avoid element inversion, the beams the springs are very long. 
Analysis Summary: 
Dim.  Type  Load  Material  Geometry  Contact 
Solver 
3D 
Static 
Force 
Linear  Nonlinear 
- 
Implicit 
Solution 
Method 
6–Arc length 
w/BFGS 
Units: 
non-dimensional 
Dimensional Data: 
L =
×
2.50 10
, 
=
×
1.00 10
−
, 
Lα =
×
2.50 10
Material Data: 
AE =
×
5.0 10
, 
1 =K
5.1
, 
=
AE L
/
(1
+
) 1.9999 10
×
=
, 
3 =K
25.0
, 
4 =K
0.1
Load: 
Axial Load 
(load values of 0.6499 10 , 1.300 10 , 1.949 10 , 2.599 10 , 3.243 10 , 1.099 10 )
×
−
×
×
×
×
0.0 varied linearly to 4.0 10
×
P =
Element Types: 
Truss (resultant) (elform=3) 
Discrete beam/cable (elform=6) 
Material Models: 
*MAT_001 or *MAT_ELASTIC 
*MAT_074 or *MAT_ELASTIC_SPRING_DISCRETE_BEAM 
Results Comparison: 
LS-DYNA displacements 
3) are compared with NAFEMS Non-Linear Benchmarks, Test NL4 for each load value. 
BU ,  CV  at locations A (Node 1), B (Node 2), and C (Node 
AU , 
NAFEMS 
NL4 
LS-DYNA 
NAFEMS 
NL4 
LS-DYNA 
NAFEMS 
NL4 
LS-DYNA 
P (load) 
AU (disp) 
AU (disp) 
BU (disp) 
BU (disp) 
CV (disp) 
CV (disp) 
0.6499 10×
650.0 
650.0 
0.0904 
0.0903 
5.241 
5.242 
1.300 10×
1300.0 
1300.0 
0.2328 
0.2329 
13.260 
13.266 
1.949 10×
1950.0 
1949.0 
0.5149 
0.5150 
27.080 
27.079 
2.599 10×
2600.0 
2600.0 
1.3440 
1.3338 
56.500 
56.500 
3.243 10×
3250.0 
3250.0 
7.0890 
7.1053 
162.600 
162.850 
-1.099 10×
3900.0 
2800.0 
4999.0 
3898.500 
41.950 
2047.200 
Figure 5.3 shows the displaced geometry at selected load values. 
These  nodal  displacement  results  (table  above  and  Figures  5.4  and  5.5  below)  were 
generated by *DATABASE_NODOUT keyword while the element stress results (Figures
Figure 5.3 – Displaced geometry at selected loads.
Figure 5.5 – Y-displacement vs. applied load for Node 3.
Figure 5.7 – Axial force resultant vs. applied load for Elements 1 and 4. 
Input deck: 
*KEYWORD 
*TITLE 
Snap-Back Under Displacement Control 
*CONTROL_IMPLICIT_AUTO 
$#   iauto    iteopt    itewin     dtmin     dtmax      
         1        20         5 1.000e-09   0.00100 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form       
         1  0.001000         2         1         2         1 
*CONTROL_IMPLICIT_SOLUTION 
$#  nsolvr    ilimit    maxref     dctol     ectol     rctol     lstol    abstol 
         6        40        15   0.00100   0.01000   0.01000  0.900000  1.000000 
$#   dnorm    diverg     istif   nlprint    
         2         1         1         2 
$#  arcctl    arcdir    arclen    arcmth    arcdmp     
         0         1       0.0         1         2 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas     
  1.000000         0       0.0       0.0       0.0 
*DATABASE_ELOUT 
$#      dt    binary 
1.0000e-04         1 
*DATABASE_GLSTAT 
$#      dt    binary 
1.0000e-04         1 
*DATABASE_MATSUM 
$#      dt    binary 
1.0000e-04         1 
*DATABASE_NODFOR 
$#      dt    binary 
1.0000e-04         1 
*DATABASE_NODOUT
$#      dt    binary 
1.0000e-04         1 
*DATABASE_BINARY_D3PLOT 
$# dt/cycl   lcdt/nr      beam     npltc    psetid 
  0.010000 
*DATABASE_NODAL_FORCE_GROUP 
$#    nsid       cid 
         1 
*DATABASE_HISTORY_BEAM 
$#    eid1      eid2      eid3      eid4       ei5      eid6      eid7      eid8 
         1         2         3         4 
*DATABASE_HISTORY_NODE 
$#    nid1      nid2      nid3      nid4       ni5      nid6      nid7      nid8 
         1         2         3         4         5 
*DEFINE_CURVE 
$#    lcid      sdir       sfa       sfo      offa      offo     dattyp 
         1         0       0.0       0.0       0.0       0.0 
$#                a1                  o1 
                 0.0                 0.0 
          1.00000000         4000.000000 
*ELEMENT_BEAM 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       5       3       0       0       0       0       0       2 
       2       2       3       2       0       0       0       0       0       2 
       3       3       2       4       0       0       0       0       0       2 
       4       4       2       1       0       0       0       0       0       2 
*NODE 
$#   nid               x               y               z      tc      rc 
       1  -1.0000000e+04             0.0             0.0 
       2             0.0             0.0             0.0 
       3     2500.000000     25.00000000             0.0 
       4     6000.000000             0.0             0.0 
       5     2500.000000     3000.000000             0.0 
*BOUNDARY_SPC_NODE 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         1         0         0         1         1         1         1         1 
*BOUNDARY_SPC_NODE 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         2         0         0         1         1         1         1         1 
         3         0         1         0         1         1         1         1 
         4         0         1         1         1         1         1         1 
         5         0         1         1         1         1         1         1 
*PART 
$# title                                                                         
Spring 1                                                                         
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1 
*SECTION_BEAM 
$#   secid    elform      shrf   qr/irid       cst     scoor      
         1         6  1.000000         0         0       0.0 
$#     vol      iner       cid        ca    offset     rrcon     srcon     trcon 
  1.000000  1.000000         0       0.0       0.0       0.0       0.0       0.0 
*MAT_ELASTIC_SPRING_DISCRETE_BEAM 
$#     mid        ro         k        f0         d       cdf       tdf        
         1  1.000000  1.500000       0.0       0.0       0.0       0.0 
$#   flcid     hlcid        c1        c2       dle     glcid      
         0         0       0.0       0.0  1.000000 
*PART 
$# title                                                                         
Truss 2                                                                          
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         2         2         2 
*SECTION_BEAM 
$#   secid    elform      shrf   qr/irid       cst     scoor      
         2         3       0.0         0         0       0.0 
$#       a       iss       itt       irr        sa         
  1.000000  1.000000  1.000000  1.000000  1.000000 
*MAT_ELASTIC
$# title                                                                         
Spring 3                                                                         
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         3         1         3 
*MAT_ELASTIC_SPRING_DISCRETE_BEAM 
$#     mid        ro         k        f0         d       cdf       tdf        
         3  1.000000  0.250000       0.0       0.0       0.0       0.0 
$#   flcid     hlcid        c1        c2       dle     glcid      
         0         0       0.0       0.0  1.000000 
*PART 
$# title                                                                         
Spring 4                                                                         
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         4         1         4 
*MAT_ELASTIC_SPRING_DISCRETE_BEAM 
$#     mid        ro         k        f0         d       cdf       tdf        
         4  1.000000  1.000000       0.0       0.0       0.0       0.0 
$#   flcid     hlcid        c1        c2       dle     glcid      
         0         0       0.0       0.0  1.000000 
*LOAD_NODE_POINT 
$#    node       dof      lcid        sf       cid        m1        m2        m3 
         1         1         1  1.000000 
*SET_NODE_LIST 
$#     sid       da1       da2       da3       da4    solver 
         1       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         1         2         3         4         5 
*END 
Notes: 
1.  Using  the  default  values  (i.e.,  BFGS  without  arc  length)  and  an  automatic  time 
stepping control, it was possible to solve the problem only  up to a certain load.  At 
this  point,  (a)  the  BFGS  solution  method  cannot  go  any  further,  due  to  the  tangent 
stiffness  matrix  becoming  close  to  null,  resulting  in  a  FATAL  ERROR  –  nonlinear 
solver  failed  to  find  equilibrium,  or  (b)  the  solution  proceeded  with  an  incorrect 
solution (no snap-back). 
2.  When the time step was allowed to increase up to 0.010, either by initial time step or 
dtmax  (automatic  time  stepping  control),  a  solution  could  be  achieved,  relatively 
quickly, but a somewhat noisy in the response. 
3.  Using the default tolerance (default=inactive) for the residual (force) norm appeared 
to result in non-convergence or inaccurate convergence (i.e. relative convergence was 
achieved, but the amount of out-of-balance forces became too large to guarantee the 
accuracy of the solution).  The tolerance on force was therefore activated and set to 
(0.010).  If this value is too large, convergence issues will result. 
4.  In  addition  to  employing  the  BFGS  solver  with  arc  length  (nsolvr=6),  it  was  found 
necessary to employ the default arc length, that is, the generalized arc length method 
(arcctl=0),  where  the  norm  of  the  global  displacement  vector  controls  the  solution; 
this  includes  all  nodes.    Attempts  at  employing  the  option  whereby  the  arc  length
6. 
Straight Cantilever Beam with Axial End Point Load 
Keywords: 
*CONTROL_IMPLICIT_AUTO 
*CONTROL_IMPLICIT_GENERAL 
*CONTROL_IMPLICIT_SOLVER 
*CONTROL_IMPLICIT_SOLUTION 
Description: 
The analysis involves a cantilever beam loaded at one end with a quasi-axial load (axial 
component=100  normal  component).    The  material  is  elastic.    The  X-displacement,  the 
Y-displacement and the Z-rotation of the end point of the beam are determined. 
A  sketch  representing  the  structure  is  shown  below  (Figure  6.1)  along  with  the  finite 
element model (Figure 6.2).
Figure 6.2 – Finite element model with applied loads and boundary conditions. 
Analysis Summary: 
Dim.  Type  Load  Material  Geometry  Contact 
Solver 
3D 
Static 
Force 
Linear  Nonlinear 
- 
Implicit 
Solution 
Method 
2-Nonlinear 
w/BFGS 
Units: 
kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) 
Dimensional Data: 
The beam has a constant square section (0.1m x 0.1m) and a total length of 3.2 m and is 
meshed with 32 beams of equal length. 
Material Data: 
Mass Density 
Young's Modulus 
Poisson's Ratio 
ρ=
=
ν =
11
×
7.85 10
×
2.10 10
0.0
/kg m
Load: 
Axial Load 
Pressure 
Element Types: 
=
3.844 10
×
=
3.844 10
×
Hughes-Liu beam with cross section integration (elform=1) 
Material Models: 
*MAT_001 or *MAT_ELASTIC 
Results Comparison: 
LS-DYNA displacements 
with NAFEMS Non-Linear Benchmarks, Test NL6. 
XU , 
YU , 
ZR  at the end  of  the beam  (Node  6)  are compared 
XU (m) 
YU (m) 
ZR (rad) 
NAFEMS NL6 
-5.0404 
-1.3472 
-3.0725 
Node 6 
-5.0629 
-1.3607 
-3.0646 
These nodal displacement results were generated by *DATABASE_NODOUT keyword.  
ZR ) histories for Node 
The X-displacement (
6  are  given  in  Figure  6.3.    Figures  6.4  and  6.5  provide  the  contour  plot  of  the  bending 
moment and the axial force, respectively, at the end of the step. 
XU ), Y-displacement (
Figure 6.3 – X-displacement, Y-displacement, and Z-rotation for Node 6.
Figure 6.5 – Contour plot of the axial force at the end of the step. 
Input deck: 
*KEYWORD 
*TITLE 
Straight Cantilever with Axial End Point Load 
*CONTROL_IMPLICIT_AUTO 
$#   iauto    iteopt    itewin     dtmin     dtmax 
         1        11         5            0.010000 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form 
         1  0.010000         2         0         2 
*CONTROL_IMPLICIT_SOLVER 
$#  lsolvr    lprint     negev     order      drcm    drcprm   autospc   autotol 
         5         2         2         0         1       0.0         1       0.0 
$#  lcpack 
         2 
*CONTROL_IMPLICIT_SOLUTION 
$#  nsolvr    ilimit    maxref     dctol     ectol     rctol     lstol    abstol 
         2        11        15    0.0010    0.0100  1.00e+10  0.900000  1.00e-10 
$#   dnorm    diverg     istif   nlprint    nlnorm 
         2         1         1         2         1 
$#  arcctl    arcdir    arclen    arcmth    arcdmp 
         6         1       0.0         1         2 
*CONTROL_OUTPUT 
$#   npopt    neecho    nrefup    iaccop     opifs    ipnint    ikedit    iflush 
         1         3         1         0       0.0         0      1000      5000 
$#   iprtf 
         3 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
  1.000000         0       0.0       0.0       0.0 
*DATABASE_NCFORC 
$#      dt    binary
0.001000         1 
*DATABASE_NODOUT 
$#      dt    binary 
  0.001000         1 
*DATABASE_NODAL_FORCE_GROUP 
$#    nsid       cid 
         2 
*DATABASE_HISTORY_NODE 
$#    nid1      nid2      nid3      nid4       ni5      nid6      nid7      nid8 
         6 
*DATABASE_HISTORY_BEAM 
$#    eid1      eid2      eid3      eid4       ei5      eid6      eid7      eid8 
         3 
*DEFINE_CURVE 
$#    lcid      sdir       sfa       sfo      offa      offo     dattyp 
         1         0  1.000000  1.000000       0.0       0.0 
$#                a1                  o1 
                 0.0                 0.0 
          1.00000000       3.8440088e+06 
*DEFINE_CURVE 
$#    lcid      sdir       sfa       sfo      offa      offo     dattyp 
         2         0  1.000000  1.000000       0.0       0.0 
$#                a1                  o1 
                 0.0                 0.0 
          1.00000000         38440.08545 
*ELEMENT_BEAM 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       1       2       3       0       0       0       0       2 
      33       1       2      92      97       0       0       0       0       2 
*NODE 
$#   nid               x               y               z      tc      rc 
       1             0.0             0.0             0.0 
      97      0.15000001             0.0      0.01000000 
*BOUNDARY_SPC_NODE 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         1         0         1         1         1         1         1         1 
*PART 
$# title                                                                         
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1 
*SECTION_BEAM 
$#   secid    elform      shrf   qr/irid       cst     scoor 
         1         1  0.830000         2         0       0.0 
$#     ts1       ts2       tt1       tt2     nsloc     ntloc 
  0.100000  0.100000  0.100000  0.100000 
*MAT_ELASTIC 
$#     mid        ro         e        pr        da        db  not used 
         1  7850.0002.1000e+11       0.0       0.0       0.0       0.0 
*LOAD_NODE_POINT 
$#    node       dof      lcid        sf       cid        m1        m2        m3 
         6         1         1 -1.000000 
*LOAD_NODE_POINT 
$#    node       dof      lcid        sf       cid        m1        m2        m3 
         6         2         2 -1.000000 
*SET_NODE_LIST_GENERATE 
$#     sid       da1       da2       da3       da4    solver 
         1       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         2        92 
*SET_NODE_LIST 
$#     sid       da1       da2       da3       da4    solver 
         2       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         6
Notes: 
1.  Using the default values, with an initial time step dt0=0.010, the problem stops at the 
12th  iteration  due  to  an energy  increase.    The  *CONTROL_IMPLICIT_GENERAL, 
*CONTROL_IMPLICIT_SOLUTION, and *CONTROL_IMPLICIT_SOLVER, with 
no  automatic  time  stepping  (*CONTROL_IMPLICIT_AUTO)  are  considered  to  be 
the default keywords. 
2.  Allowing  more  iterations  (*CONTROL_IMPLICIT_SOLUTION)  will  not  help  to 
solve the problem.  
3.  To  resolve  the  energy  increase  and  termination  stated  above,  include  the  automatic 
time stepping (*CONTROL_IMPLICIT_AUTO) entry, in particular the specification 
of dtmax.  The following situations occur when using different values of dtmax: 
dtmax  =blank  (10*dt0)  or  0.100  (these  are  actually  the  same);  the  current  step  size 
will increase right off, eventually two energy increases will occur, where time steps 
are then decreased, with the simulation then continuing until termination is reached.  
This takes the least iterations with ASCII result plots somewhat noisy. 
dtmax  =0.010  (the  initial  time  step);  solves  very  nicely  with  no  energy  increases, 
takes about 50 percent more iterations than dtmax=0.100, with smoother ASCII result 
plots. 
dtmax  =0.001  yielded  the  same  results  as  dtmax  =0.010.    dt0  appeared  to  still  be 
considered in the time step options. 
4.  It  is  also  possible  to  achieve  a  successful  solution  specifying  an  initial  time  step  of 
dt0=0.001 and a similar value for the maximum allowable time step (dtmax=0.001 in 
the *CONTROL_IMPLICIT_AUTO keyword).  Using these parameters will increase
7.  Lee’s Frame Buckling Problem 
Keywords: 
*CONTROL_IMPLICIT_AUTO 
*CONTROL_IMPLICIT_GENERAL 
*CONTROL_IMPLICIT_SOLUTION 
Description: 
The problem involves a framed structure deforming under the action of a load applied on 
one  node.    The  frame  is  pinned  to  the  ground  at  two  nodes  and  the  load  is  applied  on 
Node 56, as shown in Figure 7-1.  The finite element model is shown in Figure 7.2. 
The length of the two beams is 1.2 m.  The height of the square cross section is 0.02 m 
and the thickness is 0.03 m. 
When a certain load is reached, the structure undergoes buckling and the load-deflection 
curve shows a typical snap-back behavior, shown in Figure 7-3. 
Arc-length  method  is  required  in  order  to  capture  the  post-buckling  behavior  of  the 
structure.
Figure 7.2 – Finite element model with applied loads and boundary conditions. 
Analysis Summary: 
Dim.  Type  Load  Material  Geometry  Contact 
Solver 
3D 
Static 
Force 
Linear  Nonlinear 
- 
Implicit 
Solution 
Method 
6-Arc length 
w/BFGS 
Units: 
kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) 
Dimensional Data: 
The beam has a constant square section (0.1m x 0.1m) and a total length of 3.2 m and is
Material Data: 
Mass Density 
Young's Modulus 
Poisson's Ratio 
ρ=
=
ν =
Load: 
×
7.85 10
×
7.174 10
0.0
/kg m
10
Pa
Load is applied incrementally to the structure until buckling occurs. 
Element Types: 
Hughes-Liu beam with cross section integration (elform=1) 
Material Models: 
*MAT_001 or *MAT_ELASTIC 
Results Comparison: 
LS-DYNA displacements 
the  critical  (buckling)  load 
Test NL7. 
XU  and 
YU , at the location of the applied load (Node 56), plus 
critP ,  are  compared  with  NAFEMS  Non-Linear  Benchmarks, 
XU (m) 
NAFEMS NL7 
- 
YU (m) 
0.4884 
Node 56 
0.2620 
0.4826 
critP (N) 
1.8485 10×
1.8228 10×
These nodal displacement results were generated by *DATABASE_NODOUT keyword. 
From *DATABASE_NODOUT results, it was also seen that the critical load increment is 
at  0.364568  of  the  total  load,  which  would  therefore  correspond  to  a  load  of 
. 
critP
×
0.364568 5.0 10
1.8228 10
=
×
×
=
Figure 7.4 gives the X-displacement, Y-displacement, and resultant displacement versus
Figure 7.3 – Displaced configuration at the buckling load. 
Figure 7.4 – X-displacement, Y-displacement, and resultant
*TITLE 
Lee's Frame Buckling Problem 
*CONTROL_IMPLICIT_AUTO 
$#   iauto    iteopt    itewin     dtmin     dtmax 
         1        20         5 1.000e-09 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form 
         1  0.003000         2       100         2         1 
*CONTROL_IMPLICIT_SOLUTION 
$#  nsolvr    ilimit    maxref     dctol     ectol     rctol     lstol    abstol 
         6        30        15 1.000e-06 1.000e-05 1.000e-05  0.990000  1.000000 
$#   dnorm    diverg     istif   nlprint 
         2         1         1         2 
$#  arcctl    arcdir    arclen    arcmth    arcdmp 
         0         1       0.0         1         2 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
  1.000000         0       0.0       0.0       0.0 
*DATABASE_GLSTAT 
$#      dt    binary 
  0.001000         1 
*DATABASE_MATSUM 
$#      dt    binary 
  0.001000         1 
*DATABASE_NODFOR 
$#      dt    binary 
1.0000e-04         1 
*DATABASE_NODOUT 
$#      dt    binary 
1.0000e-04         1 
*DATABASE_BINARY_D3PLOT 
$# dt/cycl   lcdt/nr      beam     npltc    psetid 
  0.010000         0         2 
*DATABASE_NODAL_FORCE_GROUP 
$#    nsid       cid 
         1 
*DATABASE_HISTORY_NODE 
$#    nid1      nid2      nid3      nid4       ni5      nid6      nid7      nid8 
        56        36         1 
*DEFINE_CURVE 
$#    lcid      sdir       sfa       sfo      offa      offo     dattyp 
         1         0  1.000000  1.000000       0.0       0.0 
$#                a1                  o1 
                 0.0                 0.0 
          1.00000000       5.0000000e+04 
*ELEMENT_BEAM 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       1       2       3       0       0       0       0       2 
      31       1      32      56      61       0       0       0       0       2 
*NODE 
$#   nid               x               y               z      tc      rc 
       1             0.0             0.0             0.0 
      61      0.17999999      1.20000005      0.10000000 
*BOUNDARY_SPC_NODE 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         1         0         1         1         1         1         1 
*BOUNDARY_SPC_NODE 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
        36         0         1         1         1         1         1 
*PART 
$# title                                                                         
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1
$#   secid    elform      shrf   qr/irid       cst     scoor 
         1         1  0.830000         5         0       0.0 
$#     ts1       ts2       tt1       tt2     nsloc     ntloc 
  0.030000  0.030000      0.02      0.02 
*MAT_ELASTIC 
$#     mid        ro         e        pr        da        db  not used 
         1  7850.0007.1740e+10       0.0       0.0       0.0       0.0 
*LOAD_NODE_POINT 
$#    node       dof      lcid        sf       cid        m1        m2        m3 
        56         2         1 -1.000000 
*SET_NODE_LIST 
$#     sid       da1       da2       da3       da4    solver 
         1       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         1         6        36        56 
*END
8. 
Pin-Ended Double Cross: In-Plane Vibration 
Keywords: 
*CONTROL_IMPLICIT_AUTO 
*CONTROL_IMPLICIT_EIGENVALUE 
*CONTROL_IMPLICIT_GENERAL 
*CONTROL_IMPLICIT_SOLVER 
Description: 
This example shows the behavior of beam elements in a modal analysis.  The structure is 
a  double  cross  pinned  to  the  ground  as  show  in  Figure  8.1.    All  inner  nodes  have 
= .  On the outer nodes 
= . 
=
=
=
=
=
=
The finite element model is shown in Figure 8.2. 
The problem requires the extraction of numerically close eigenvalues, making it an ideal 
benchmark to check the element formulation accuracy. 
Each arm of the cross is modeled with 4 beams, for a total of 32 beams.  The length of 
each arm is 5 m.
Figure 8.2 – Finite element model with end point boundary conditions. 
Analysis Summary: 
Dim.  Type  Load  Material  Geometry  Contact 
Solver 
3D  Modal 
- 
Linear 
Linear 
- 
Implicit 
Solution 
Method 
Block Shift 
and Inverted 
Lanczos 
Units: 
kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) 
Dimensional Data:
Material Data: 
Mass Density 
Young's Modulus 
Poisson's Ratio 
ρ=
=
ν =
Element Types: 
11
×
8.00 10
×
2.00 10
0.3
/kg m
Pa
Hughes-Liu beam with cross section integration (elform=1) 
Belytschko-Schwer resultant beam (elform=2) 
Small displacement, linear Timoshenko beam with exact stiffness (elform=13) 
Material Models: 
*MAT_001 or *MAT_ELASTIC 
Results Comparison: 
LS-DYNA  natural  frequencies,  first  16  (frequency  in  Hertz),  and  mode  shapes  (first  6) 
are compared with Standard NAFEMS Benchmarks, Test FV2. 
Mode(s) 
NAFEMS  
FV2 (Hz) 
Hughes-Liu 
Beam (Hz) 
Belytschko-
Schwer Beam 
Timoshenko 
Beam (Hz) 
1 
2, 3 
11.336 
11.641 
11.323 
11.365 
17.709 
19.080 
17.621 
17.803 
4, 5, 6, 7, 8 
17.709 
19.115 
17.649 
17.832 
9 
45.345 
51.691 
44.833 
45.620 
10, 11 
57.390 
73.717 
55.673 
57.399 
 12, 13, 14, 15, 16 
57.390 
74.381 
55.952
As seen in the results, using the LS-DYNA default beam (Hughes-Liu - elform=1) results 
in poor accuracy in the frequency calculation due to its omission of the first (no bending) 
and second (no rotary inertia) order terms (more elements are often needed in an attempt 
to  overcome  this  limitation).    The  Hughes-Liu  beam  effectively  generates  a  constant 
moment  along  its  length,  so,  as  with  brick  and  shell  elements,  meshes  need  to  be 
reasonably fine to achieve adequate accuracy. 
The  Belytschko-Schwer  beam  (elform=2)  provides  good  frequency  results  throughout 
most  of  the  range  covered,  with  some  minor  differences  at  the  higher  frequency  range.  
This element is often acceptable. 
The Timoshenko beam (elform=13), with its inclusion of second order (rotary inertia and 
shear  distortion)  terms,  provides  very  good  results  throughout  the  reported  frequency 
range.    This  element  formulation  is  generally  recommended  for  this  type  of  frequency 
analysis. 
Eigenvalue Results: 
From  the  eigout  file,  generated  by  the  *CONTROL_IMPLICIT_EIGENVALUE 
keyword: 
Hughes-Liu beam (elform=1): 
Pin-Ended Double Cross: In-Plane Vibration                               
r e s u l t s   o f   e i g e n v a l u e   a n a l y s i s: 
                             |------ frequency -----| 
        MODE    EIGENVALUE       RADIANS        CYCLES        PERIOD 
           1   5.349990E+03   7.314363E+01   1.164117E+01   8.590202E-02 
           2   1.437182E+04   1.198825E+02   1.907989E+01   5.241119E-02 
           3   1.437182E+04   1.198825E+02   1.907989E+01   5.241119E-02 
           4   1.442423E+04   1.201009E+02   1.911465E+01   5.231589E-02 
           5   1.442423E+04   1.201009E+02   1.911465E+01   5.231589E-02 
           6   1.442423E+04   1.201009E+02   1.911465E+01   5.231589E-02 
           7   1.442423E+04   1.201009E+02   1.911465E+01   5.231589E-02 
           8   1.442423E+04   1.201009E+02   1.911465E+01   5.231589E-02 
           9   1.054860E+05   3.247862E+02   5.169132E+01   1.934561E-02 
          10   2.145341E+05   4.631783E+02   7.371711E+01   1.356537E-02 
          11   2.145341E+05   4.631783E+02   7.371711E+01   1.356537E-02 
          12   2.184158E+05   4.673498E+02   7.438102E+01   1.344429E-02 
          13   2.184158E+05   4.673498E+02   7.438102E+01   1.344429E-02 
          14   2.184158E+05   4.673498E+02   7.438102E+01   1.344429E-02 
          15   2.184158E+05   4.673498E+02   7.438102E+01   1.344429E-02
Belytschko-Schwer beam (elform=2): 
Pin-Ended Double Cross: In-Plane Vibration                               
r e s u l t s   o f   e i g e n v a l u e   a n a l y s i s: 
                             |------ frequency -----| 
        MODE    EIGENVALUE       RADIANS        CYCLES        PERIOD 
           1   5.061497E+03   7.114420E+01   1.132295E+01   8.831620E-02 
           2   1.225757E+04   1.107139E+02   1.762066E+01   5.675155E-02 
           3   1.225757E+04   1.107139E+02   1.762066E+01   5.675155E-02 
           4   1.229691E+04   1.108915E+02   1.764892E+01   5.666068E-02 
           5   1.229691E+04   1.108915E+02   1.764892E+01   5.666068E-02 
           6   1.229691E+04   1.108915E+02   1.764892E+01   5.666068E-02 
           7   1.229691E+04   1.108915E+02   1.764892E+01   5.666068E-02 
           8   1.229691E+04   1.108915E+02   1.764892E+01   5.666068E-02 
           9   7.935148E+04   2.816939E+02   4.483298E+01   2.230501E-02 
          10   1.223614E+05   3.498019E+02   5.567270E+01   1.796212E-02 
          11   1.223614E+05   3.498019E+02   5.567270E+01   1.796212E-02 
          12   1.235904E+05   3.515543E+02   5.595161E+01   1.787259E-02 
          13   1.235904E+05   3.515543E+02   5.595161E+01   1.787259E-02 
          14   1.235904E+05   3.515543E+02   5.595161E+01   1.787259E-02 
          15   1.235904E+05   3.515543E+02   5.595161E+01   1.787259E-02 
          16   1.235904E+05   3.515543E+02   5.595161E+01   1.787259E-02 
Timoshenko beam (elform=13): 
Pin-Ended Double Cross: In-Plane Vibration 
r e s u l t s   o f   e i g e n v a l u e   a n a l y s i s: 
                             |------ frequency -----| 
        MODE    EIGENVALUE       RADIANS        CYCLES        PERIOD 
           1   5.099519E+03   7.141092E+01   1.136540E+01   8.798634E-02 
           2   1.251262E+04   1.118598E+02   1.780305E+01   5.617016E-02 
           3   1.251262E+04   1.118598E+02   1.780305E+01   5.617016E-02 
           4   1.255348E+04   1.120423E+02   1.783209E+01   5.607869E-02 
           5   1.255348E+04   1.120423E+02   1.783209E+01   5.607869E-02 
           6   1.255348E+04   1.120423E+02   1.783209E+01   5.607869E-02 
           7   1.255348E+04   1.120423E+02   1.783209E+01   5.607869E-02 
           8   1.255348E+04   1.120423E+02   1.783209E+01   5.607869E-02 
           9   8.216358E+04   2.866419E+02   4.562048E+01   2.191998E-02 
          10   1.300676E+05   3.606489E+02   5.739905E+01   1.742189E-02 
          11   1.300676E+05   3.606489E+02   5.739905E+01   1.742189E-02 
          12   1.314649E+05   3.625808E+02   5.770653E+01   1.732906E-02 
          13   1.314649E+05   3.625808E+02   5.770653E+01   1.732906E-02 
          14   1.314649E+05   3.625808E+02   5.770653E+01   1.732906E-02 
          15   1.314649E+05   3.625808E+02   5.770653E+01   1.732906E-02 
          16   1.314649E+05   3.625808E+02   5.770653E+01   1.732906E-02 
Mode Shapes (first six): 
From the d3plot file, generated by the *DATABASE_BINARY_D3PLOT keyword, the 
user  can  obtain  the  first  six  mode  shapes  (stick  view)  for  the  Hughes-Li  beam  (Figure 
8.3), the Belytschko-Schwer Beam (Figure 8.4), and the Timoshenko beam (Figure 8.5). 
Displacement contouring of the first six mode shapes are given in Figures 8.6, 8.7, and
Figure 8.3 - Mode shapes for Hughes-Liu beam (stick view).
Figure 8.5 - Mode shapes for Timoshenko beam (stick view).
Figure 8.7 - Mode shapes for Belytschko beam (displacement contouring).
*TITLE 
Pin-Ended Double Cross: In-Plane Vibration 
*CONTROL_IMPLICIT_AUTO 
$#   iauto    iteopt    itewin     dtmin     dtmax 
         1        11        15       0.0       0.0 
*CONTROL_IMPLICIT_EIGENVALUE 
$#    neig    center     lflag    lftend     rflag    rhtend    eigmth    shfscl 
        16    11.000         0 -1.00e+29         0  1.00e+29         2       0.0 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form 
         1  1.00e-04         2         1         2 
*CONTROL_IMPLICIT_SOLVER 
$#  lsolvr    lprint     negev     order      drcm    drcprm   autospc   autotol 
        16         1         1         0         1       0.0         1       0.0 
*DATABASE_BINARY_D3PLOT 
$# dt/cycl   lcdt/nr      beam     npltc    psetid 
  0.010000         0         2 
*ELEMENT_BEAM 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       1       2       3       0       0       0       0       2 
      32       1      61      74      76       0       0       0       0       2 
*NODE 
$#   nid               x               y               z      tc      rc 
       1             0.0             0.0             0.0 
      76      2.79029131     -2.20970869      1.00000000 
*BOUNDARY_SPC_SET 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         2         0         1         1         1         1         1         0 
*BOUNDARY_SPC_SET 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         1         0         0         0         1         1         1         0 
*PART 
$# title                                                                         
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1 
*SECTION_BEAM 
$#   secid    elform      shrf   qr/irid       cst     scoor 
         1         1  0.833333       2.0       0.0       0.0 
$#     ts1       ts2       tt1       tt2     nsloc     ntloc 
  0.125000  0.125000  0.125000  0.125000       0.0       0.0 
$$#   secid    elform      shrf   qr/irid       cst     scoor 
$         1         2  0.833333         2         0       0.0 
$$#       a       iss       itt         j        sa       ist 
$ 0.01562502.0345e-052.0345e-054.0690e-050.01302083 
$$#   secid    elform      shrf   qr/irid       cst     scoor 
$         1        13  0.833333         2         0       0.0 
$$#       a       iss       itt         j        sa       ist 
$ 0.01562502.0345e-052.0345e-054.0690e-050.01302083 
*MAT_ELASTIC 
$#     mid        ro         e        pr        da        db  not used 
         1  8000.0002.0000e+11  0.300000       0.0       0.0       0.0 
*SET_NODE_LIST_GENERATE 
$#     sid       da1       da2       da3       da4    solver 
         1       0.0       0.0       0.0       0.0 
$#   b1beg     b1end     b2beg     b2end     b3beg     b3end     b4beg     b4end 
         2         4         6        24        27        29        31        42 
        44        46        48        59        61        63        65        76 
*SET_NODE_LIST 
$#     sid       da1       da2       da3       da4    solver 
         2       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         1         5        30        47        64        60        43        26
Notes: 
1.  The  main  difference  among  these  element  formulations  is  the  inclusion  of  different 
second  order  terms  for  rotary  inertia  and  shear  distortion.    The  Euler  (Belytschko-
Schwer)  beam  model  includes  only  the  first  order  terms,  lateral  displacement  and 
bending  moment.    The  simple  shear  (Hughes-Liu)  beam  model  includes  only  the 
translation first order term (no bending) plus shear distortion, while the Timoshenko 
beam  model  includes  both  rotary  inertia  and  shear  distortion  in  addition  to  the  first
9.  Simply Supported Thin Annular Plate (coarse mesh) 
Keyword: 
*CONTROL_IMPLICIT_EIGENVALUE 
*CONTROL_IMPLICIT_GENERAL 
Description: 
A  simply-supported  annular  plate  of  thickness  t=0.06  m  is  to  be  analyzed  to  determine 
the first nine natural frequencies.  The inner radius is 1.8 m and the outer radius is 6.0 m.  
This coarse mesh analysis has 26 shell elements (circumferential) by 3 elements (radial).  
All nodes have 
= .  On the outer nodes 
=
=
ZU = . 
A  sketch  representing  the  structure  is  shown  below  (Figure  9.1)  along  with  the  finite 
element model (Figure 9.2).
Figure 9.2 – Coarse mesh finite element model with simply supported 
boundary conditions on outer nodes. 
Analysis Summary: 
Dim.  Type  Load  Material  Geometry  Contact 
Solver 
3D  Modal 
- 
Linear 
Linear 
- 
Implicit 
Solution 
Method 
Block Shift 
and Inverted 
Lanczos 
Units: 
kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) 
Dimensional Data: 
ro
6=
, 
ri
8.1=
, 
06.0=
Material Data: 
Mass Density 
Young's Modulus 
Poisson's Ratio 
ρ=
=
ν =
Element Types: 
11
×
8.00 10
×
2.00 10
0.3
/kg m
Pa
Fully integrated shell (elform=16) 
Material Models: 
*MAT_001 or *MAT_ELASTIC 
Results Comparison: 
LS-DYNA  natural  frequencies,  first  10  (frequency  in  Hertz),  and  mode  shapes  (first  5) 
are compared with NAFEMS Natural Frequency Benchmark NF14. 
Mode(s) 
NAFEMS NF14 (Hz) 
Coarse Mesh (Hz) 
1 
2, 3 
4, 5 
6 
7, 8 
9, 10 
1.870 
5.137 
9.673 
14.850 
15.570 
18.380 
1.806 
5.423 
10.179 
13.217 
16.239 
16.691 
It  is  seen  that  even  with  this  rather  coarse  mesh  refinement,  the  LS-DYNA  natural 
frequency results provide a fair comparison with the NAFEMS Selected Benchmarks for
Eigenvalue Results: 
From  the  eigout  file,  generated  by  the  *CONTROL_IMPLICIT_EIGENVALUE 
keyword: 
Simply Supported Thin Annular Plate (coarse mesh) 
r e s u l t s   o f   e i g e n v a l u e   a n a l y s i s: 
                             |------ frequency -----| 
        MODE    EIGENVALUE       RADIANS        CYCLES        PERIOD 
           1   1.287078E+02   1.134495E+01   1.805604E+00   5.538311E-01 
           2   1.161053E+03   3.407423E+01   5.423083E+00   1.843970E-01 
           3   1.161053E+03   3.407423E+01   5.423083E+00   1.843970E-01 
           4   4.090826E+03   6.395957E+01   1.017948E+01   9.823683E-02 
           5   4.090827E+03   6.395957E+01   1.017948E+01   9.823683E-02 
           6   6.896060E+03   8.304252E+01   1.321663E+01   7.566227E-02 
           7   1.041122E+04   1.020354E+02   1.623944E+01   6.157849E-02 
           8   1.041122E+04   1.020354E+02   1.623944E+01   6.157848E-02 
           9   1.099787E+04   1.048707E+02   1.669070E+01   5.991361E-02 
          10   1.099787E+04   1.048707E+02   1.669070E+01   5.991361E-02 
Mode Shapes (first five): 
Figures 9.3, 9.4, and 9.5 show the first 5 mode shapes with no contouring while Figures 
9.6. 9.7, and 9.8 show the same 5 mode shapes with displacement contouring.
Figure 9.4 - Modes 2 and 3, 5.423 Hz (NAFEMS 5.137) - no contouring.
Figure 9.6 - Mode 1, 1.806 Hz (NAFEMS 1.870) - displacement contouring.
Figure 9.8 - Modes 4 and 5, 10.179 Hz (NAFEMS 9.673) - displacement contouring. 
64
*TITLE 
Simply Supported Thin Annular Plate (coarse mesh) 
*CONTROL_IMPLICIT_EIGENVALUE 
$#    neig    center     lflag    lftend     rflag    rhtend    eigmth    shfscl 
        10       0.0         1  1.000000         1  30.00000         2       0.0 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form 
         1  1.000000 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
  1.000000         0       0.0       0.0       0.0 
*DATABASE_BINARY_D3PLOT 
$# dt/cycl   lcdt/nr      beam     npltc    psetid 
  1.000000 
*ELEMENT_SHELL 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       1      27      28       2 
      78       1      78     104      79      53 
*NODE 
$#   nid               x               y               z      tc      rc 
       1      1.79999995             0.0             0.0 
     104      5.82565355     -1.43588233             0.0       3       1 
*BOUNDARY_SPC_SET 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         1         0         1         1         1         0         0         1 
*BOUNDARY_SPC_SET 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         2         0         1         1         0         0         0         1 
*PART 
$# title                                                                         
material type # 1  (Elastic)                                                     
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1 
*SECTION_SHELL 
$#   secid    elform      shrf       nip     propt   qr/irid     icomp     setyp 
         1        16       0.0         0         1       0.0         0         1 
$#      t1        t2        t3        t4      nloc     marea 
  0.060000  0.060000  0.060000  0.060000         0       0.0 
*MAT_ELASTIC 
$#     mid        ro         e        pr        da        db  not used 
         1  8000.0002.0000e+11  0.300000       0.0       0.0       0.0 
*SET_NODE_LIST_GENERATE 
$#     sid       da1       da2       da3       da4    solver 
         1       0.0       0.0       0.0       0.0 
$#   b1beg     b1end     b2beg     b2end     b3beg     b3end     b4beg     b4end 
        79       104 
*SET_NODE_LIST_GENERATE 
$#     sid       da1       da2       da3       da4    solver 
         2       0.0       0.0       0.0       0.0 
$#   b1beg     b1end     b2beg     b2end     b3beg     b3end     b4beg     b4end 
         1        78 
*END
10.  Simply Supported Thin Annular Plate (fine mesh) 
Keyword: 
*CONTROL_IMPLICIT_EIGENVALUE 
*CONTROL_IMPLICIT_GENERAL 
Description: 
A  simply-supported  annular  plate  of  thickness  t=0.06  m  is  to  be  analyzed  to  determine 
the first nine natural frequencies.  The inner radius is 1.8 m and the outer radius is 6.0 m.  
This  fine  mesh  analysis  has  32  shell  elements  (circumferential)  by  5  elements  (radial).  
All nodes have 
= .  On the outer nodes 
=
=
ZU = . 
A  sketch  representing  the  structure  is  shown  below  (Figure  10.1)  along  with  the  finite 
element model (Figure 10.2).
Figure 10.2 – Fine mesh finite element model with simply supported 
boundary conditions on outer nodes. 
Analysis Summary: 
Dim.  Type  Load  Material  Geometry  Contact 
Solver 
3D  Modal 
- 
Linear 
Linear 
- 
Implicit 
Solution 
Method 
Block Shift 
and Inverted 
Lanczos 
Units: 
kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) 
Dimensional Data: 
ro
6=
, 
ri
8.1=
, 
06.0=
Material Data: 
Mass Density 
Young's Modulus 
Poisson's Ratio 
ρ=
=
ν =
Element Types: 
11
×
8.00 10
×
2.00 10
0.3
/kg m
Pa
Fully integrated shell (elform=16) 
Material Models: 
*MAT_001 or *MAT_ELASTIC 
Results Comparison: 
LS-DYNA  natural  frequencies,  first  10  (frequency  in  Hertz),  and  mode  shapes  (first  5) 
are compared with NAFEMS Natural Frequency Benchmark NF14. 
Mode(s) 
NAFEMS NF14 (Hz) 
Fine Mesh (Hz) 
1 
2, 3 
4, 5 
6 
7, 8 
9, 10 
1.870 
5.137 
9.673 
14.850 
15.570 
18.380 
1.867 
5.197 
9.801 
14.471 
15.665 
17.798 
It  is  seen  that  with  only  a  slight  increase  in  mesh  refinement,  the  LS-DYNA  natural 
frequency  results  compare  nicely  with  the  NAFEMS  Selected  Benchmarks  for  Natural
Eigenvalue Results: 
From  the  eigout  file,  generated  by  the  *CONTROL_IMPLICIT_EIGENVALUE 
keyword: 
Simply Supported Thin Annular Plate (fine mesh) 
r e s u l t s   o f   e i g e n v a l u e   a n a l y s i s: 
                             |------ frequency -----| 
        MODE    EIGENVALUE       RADIANS        CYCLES        PERIOD 
           1   1.377019E+02   1.173465E+01   1.867627E+00   5.354388E-01 
           2   1.066283E+03   3.265399E+01   5.197045E+00   1.924171E-01 
           3   1.066283E+03   3.265399E+01   5.197045E+00   1.924171E-01 
           4   3.791946E+03   6.157878E+01   9.800567E+00   1.020349E-01 
           5   3.791946E+03   6.157878E+01   9.800567E+00   1.020349E-01 
           6   8.267193E+03   9.092411E+01   1.447102E+01   6.910362E-02 
           7   9.688143E+03   9.842836E+01   1.566536E+01   6.383511E-02 
           8   9.688143E+03   9.842836E+01   1.566536E+01   6.383511E-02 
           9   1.250545E+04   1.118278E+02   1.779794E+01   5.618626E-02 
          10   1.250545E+04   1.118278E+02   1.779794E+01   5.618626E-02 
Mode Shapes (first three): 
Figures  10.3,  10.4,  and  10.5  show  the  first  5  mode  shapes  with  no  contouring  while 
Figures 10.6. 10.7, and 10.8 show the same 5 mode shapes with displacement contouring.
Figure 10.4 - Modes 2 and 3, 5.197 Hz (NAFEMS 5.137) - no contouring.
Figure 10.6 - Mode 1, 1.867 Hz (NAFEMS 1.870) - displacement contouring.
Figure 10.8 - Modes 4 and 5, 9.801 Hz (NAFEMS 9.673) - displacement contouring. 
72
*TITLE 
Simply Supported Thin Annular Plate (fine mesh) 
*CONTROL_IMPLICIT_EIGENVALUE 
$#    neig    center     lflag    lftend     rflag    rhtend    eigmth    shfscl 
        10       0.0         1  1.000000         1  30.00000         2       0.0 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form 
         1  1.000000 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
  1.000000         0       0.0       0.0       0.0 
*DATABASE_BINARY_D3PLOT 
$# dt/cycl   lcdt/nr      beam     npltc    psetid 
  1.000000 
*ELEMENT_SHELL 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       1      33      34       2 
     192       1     192     224     193     161 
*NODE 
$#   nid               x               y               z      tc      rc 
       1      1.79999995             0.0             0.0 
     224      5.88471174     -1.17054188             0.0       3       1 
*BOUNDARY_SPC_SET 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         1         0         1         1         1         0         0         1 
*BOUNDARY_SPC_SET 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         2         0         1         1         0         0         0         1 
*PART 
$# title                                                                         
material type # 1  (Elastic)                                                     
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1 
*SECTION_SHELL 
$#   secid    elform      shrf       nip     propt   qr/irid     icomp     setyp 
         1         6       0.0         0         1       0.0         0         1 
$#      t1        t2        t3        t4      nloc     marea 
  0.060000  0.060000  0.060000  0.060000         0       0.0 
*MAT_ELASTIC 
$#     mid        ro         e        pr        da        db  not used 
         1  8000.0002.0000e+11  0.300000       0.0       0.0       0.0 
*SET_NODE_LIST_GENERATE 
$#     sid       da1       da2       da3       da4    solver 
         1       0.0       0.0       0.0       0.0 
$#   b1beg     b1end     b2beg     b2end     b3beg     b3end     b4beg     b4end 
       193       224 
*SET_NODE_LIST_GENERATE 
$#     sid       da1       da2       da3       da4    solver 
         2       0.0       0.0       0.0       0.0 
$#   b1beg     b1end     b2beg     b2end     b3beg     b3end     b4beg     b4end 
         1       192 
*END
11.  Transient Response to a Constant Force 
Keyword: 
*CONTROL_IMPLICIT_DYNAMICS 
*CONTROL_IMPLICIT_GENERAL 
*CONTROL_IMPLICIT_SOLVER 
*CONTROL_IMPLICIT_SOLUTION 
Description: 
A  mass  m=25.9067  lbf-s2/in  is  attached  in  the  middle  of  a  steel  beam  of  length  l=240 
inches and geometric properties shown below.  The beam is subjected to a dynamic load 
F(t)  with  a  rise  time  of  0.075  seconds  and  a  maximum  constant  value  of  2000  pound-
force.  The weight of the beam is considered negligible.  Determine the time of maximum 
displacement response tmax and the maximum displacement response ymax.  Additionally, 
bendσ  in the beam.  The attached mass is modeled 
determine the maximum bending stress 
with a lumped mass element at the central node of the beam. 
A  sketch  representing  the  structure  is  shown  below  (Figure  11.1)  along  with  the  finite 
element model (Figure 11.2).
Figure 11.2 – Finite element model with applied load (Node 12) 
and boundary conditions.  In-plane boundary conditions and 
lumped mass (Node 12) are not shown. 
Analysis Summary: 
Dim. 
Type 
Load  Material  Geometry  Contact 
Solver 
3D  Dynamic  Force 
Linear 
Linear 
- 
Implicit 
Solution 
Method 
2-Nonlinear 
w/BFGS 
Units: 
lbf-s2/in, in, s, lbf, psi, lbf-in (blob, inch, second, pound force, pound force/inch2, 
pound force-inch) 
Dimensional Data: 
=
240.0
in
, 
=
18.0
in
, 
zI
=
800.6
in
As  a  cross-section-integrated  beam  is  used,  the  cross  sectional  dimension  is  calculated.  
, a thickness of 
Given 
 is obtained. 
800.6
1.647
 and 
18.0
in
in
in
=
=
=
Material Data: 
Mass Density 
Young's Modulus 
Poisson's Ratio 
Nodal Mass 
=
=
ν =
=
Load: 
−
20
lbf
−
/
in
×
1.0 10
×
3.0 10
0.3
25.9067
psi
blobs
Lateral Load 
F t =
( ) *DEFINE_CURVE
Element Types: 
Hughes-Liu beam with cross section integration (elform=1) 
Lumped mass (*ELEMENT_MASS entry) 
Material Models: 
*MAT_001 or *MAT_ELASTIC 
Results Comparison: 
LS-DYNA  results  for  time  of  the  maximum  displacement  response  tmax,  the  maximum 
σ   in  the  beam  are 
displacement  response  ymax,  and  the  maximum  bending  stress 
compared with J.M. Biggs' studies in Introduction to Structural Dynamics (pg. 50). 
bend
Time - tmax (s) 
Disp. - ymax (in) 
Stress - 
σ  (psi) 
bend
Biggs 
0.0920 
0.3310 
1.8600 10×
Node 12/Element 10 
0.0930 
0.3421 
1.8151 10×
These  nodal  time/displacement  results  (Figure  11.3)  were  generated  by  *DATABASE_ 
NODOUT  keyword  while  the  element  stress  results  (Figure  11.4)  were  generated  by 
*DATABASE_ELOUT.
Lobatto integration (qr=4 - 3×3 quadrature - *SECTION_BEAM) was employed since it 
has an advantage in that the inner and outer integration points are on the beam surfaces.  
Gauss  integration  is  the  default  quadrature  rule  (qr=2  -  2×2  quadrature  -  *SECTION_ 
BEAM). 
The  contour  plots  of  the  axial  beam  stresses  for  the  upper  (ip=1)  and  lower  (ip=3) 
surfaces of the beam (Figure 11.5) were obtained from the d3plot file at t=0.093 s which 
were generated by the *DATABASE_BINARY_D3PLOT keyword.
Figure 11.4 – Axial beam stress vs. time at the upper (ip=1), the point of maximum 
bending stress, and the lower (ip=3) beam surfaces for Element 10. 
Figure 11.5 – Contour plots of the axial beam stresses for the upper (ip=1)
*TITLE 
Transient Response to a Constant Force 
*CONTROL_IMPLICIT_DYNAMICS 
$#   imass     gamma      beta 
         1  0.500000  0.250000 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form 
         1  0.001000         2         1         2 
*CONTROL_IMPLICIT_SOLVER 
$#  lsolvr    lprint     negev     order      drcm    drcprm   autospc   autotol 
         4         2         2         0         1       0.0         1       0.0 
$#  lcpack 
         2 
*CONTROL_IMPLICIT_SOLUTION 
$#  nsolvr    ilimit    maxref     dctol     ectol     rctol     lstol    abstol 
         2        11        15    0.0010    0.0100  1.00e+10  0.900000  1.00e-10 
$#   dnorm    diverg     istif   nlprint 
         2         1         1         2 
$#  arcctl    arcdir    arclen    arcmth    arcdmp 
         0         1       0.0         1         2 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
  0.100000         0  0.900000       0.0       0.0 
*DATABASE_ELOUT 
$#      dt    binary 
1.0000e-05         1 
*DATABASE_MATSUM 
$#      dt    binary 
1.0000e-05         1 
*DATABASE_NODOUT 
$#      dt    binary 
1.0000e-05         1 
*DATABASE_SPCFORC 
$#      dt    binary 
1.0000e-05         1 
*DATABASE_BINARY_D3PLOT 
$# dt/cycl   lcdt/nr      beam     npltc    psetid 
1.0000e-05 
*DATABASE_BINARY_D3THDT 
$# dt/cycl   lcdt/nr      beam     npltc    psetid 
2.0000e-04 
*DATABASE_EXTENT_BINARY 
$#   neiph     neips    maxint    strflg    sigflg    epsflg    rltflg    engflg 
         0         0         0         0         1         1         1         1 
$#  cmpflg    ieverp    beamip     dcomp      shge     stssz    n3thdt   ialemat 
         0         0        20         1         1         1         2 
*DATABASE_HISTORY_NODE 
$#    nid1      nid2      nid3      nid4       ni5      nid6      nid7      nid8 
        12         1         2 
*DATABASE_HISTORY_BEAM 
$#    eid1      eid2      eid3      eid4       ei5      eid6      eid7      eid8 
        10        11 
*DEFINE_CURVE 
$#    lcid      sdir       sfa       sfo      offa      offo     dattyp 
         1         0  1.000000  1.000000       0.0       0.0 
$#                a1                  o1 
                 0.0                 0.0 
          0.07500000       2.0000000e+04 
          1.00000000       2.0000000e+04 
*ELEMENT_BEAM 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       1       3      22 
      20       1      21       2      41 
*ELEMENT_MASS 
$#   eid      id            mass     pid
1             0.0             0.0             0.0 
      41     234.0000000             0.0      0.99996525 
*BOUNDARY_SPC_SET 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         2         0         1         1         1         1         1 
*BOUNDARY_SPC_SET 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         3         0         0         0         1         1         1 
*PART 
$# title                                                                         
Part          1 for Mat         1 and Elem Type         1                        
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1 
*SECTION_BEAM 
$#   secid    elform      shrf   qr/irid       cst     scoor 
         1         1  0.830000         4         0       0.0 
$#     ts1       ts2       tt1       tt2     nsloc     ntloc 
  1.647220  1.647220      18.0      18.0 
*MAT_ELASTIC 
$#     mid        ro         e        pr        da        db  not used 
         11.0000e-203.0000e+07  0.300000       0.0       0.0       0.0 
*LOAD_NODE_SET 
$#    nsid       dof      lcid        sf       cid        m1        m2        m3 
         1         2         1  1.000000 
*SET_NODE_LIST 
$#     sid       da1       da2       da3       da4    solver 
         1       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
        12 
*SET_NODE_LIST 
$#     sid       da1       da2       da3       da4    solver 
         2       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         1         2 
*SET_NODE_LIST 
$#     sid       da1       da2       da3       da4    solver 
         3       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         3         4         5         6         7         8         9        10 
        11        12        13        14        15        16        17        18 
        19        20        21        22        23        24        25        26 
        27        28        29        30        31        32        33        34 
        35        36        37        38        39        40        41 
*END
12.  Simply Supported Square Plate: Out-of-Plane Vibration 
(solid mesh) 
Keywords: 
*CONTROL_IMPLICIT_EIGENVALUE 
*CONTROL_IMPLICIT_GENERAL 
Description: 
Determine the first 10 natural frequencies of a solid simply-supported plate of thickness 
t=1.0  m.    Each  side  of  the  plate  measure  10.0  m.    The  plate  is  meshed  with  solid 
hexahedra  element  with  an  8  x  8  x  3  density.    On  the  lower  surface,  outer  boundary 
nodes, 
ZU = . 
The finite element model is shown in Figure 12.1. 
Figure 12.1 – Finite element model with simply supported
Analysis Summary: 
Dim.  Type  Load  Material  Geometry  Contact 
Solver 
3D  Modal 
- 
Linear 
Linear 
- 
Implicit 
Solution 
Method 
Block Shift 
and Inverted 
Lanczos 
Units: 
kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) 
Dimensional Data: 
Rectangular dimensions of square plate: 10.0 m x 10.0 m x 1.00 m. 
Material Data: 
Mass Density 
Young's Modulus 
Poisson's Ratio 
ρ=
=
ν =
Element Types: 
11
×
8.00 10
×
2.00 10
0.3
/kg m
Pa
Constant stress solid (elform=1) 
Fully integrated S/R solid (elform=2) 
Fully integrated S/R solid - for poor aspect ratio (eff) - (elform=-1) 
Fully integrated S/R solid - for poor aspect ratio (acc) - (elform=-2) 
Fully integrated quadratic 8 node element with nodal rotations (elform=3) 
Material Models: 
*MAT_001 or *MAT_ELASTIC 
Results Comparison: 
LS-DYNA natural frequencies, first 10 (frequency in Hertz), and mode shapes (4 through
Mode(s) 
NAFEMS 
FV52 (Hz) 
elform=1 
(Hz) 
elform=2 
(Hz) 
elform=-1 
(Hz) 
elform=-2 
(Hz) 
elform=3 
(Hz) 
1, 2, 3 
rigid body 
rigid body 
rigid body 
rigid body 
rigid body 
rigid body 
4 
45.897 
44.040 
48.508 
45.448 
46.2060 
43.370 
5, 6 
109.440 
106.468 
120.388 
107.114 
109.265 
104.703 
7 
8 
9 
167.890 
155.523 
169.601 
159.102 
163.943 
153.862 
193.590 
193.582 
193.526 
193.518 
193.526 
193.227 
206.190 
200.135 
200.188 
198.791 
200.176 
196.485 
10 
206.190 
200.135 
200.188 
198.873 
200.176 
197.280 
Hourglass control (*HOURGLASS) is necessary for the constant stress solid (elform=1) 
element formulation (the LS-DYNA default), especially at higher frequencies.  Only this 
element formulation (elform=1) makes use of this feature 
The  constant  stress  solid  (elform=1),  the  fully  integrated  S/R  solid  (elform=2),  and  the 
fully  integrated  quadratic  8  node  element  with  nodal  rotations  (elform=3)  all  provide 
similar frequency results for this analysis. 
The  fully  integrated  quadratic  8  node  element  with  nodal  rotations  (elform=3) 
formulation  provides two distinct modes and  frequencies for  modes 9 and  10,  whereas, 
all the other formulations provide the same results for modes 9 and 10.  This is perhaps 
due to the accountability of the nodal rotations. 
The  aspect  ratio  of  these  elements  is  3.75  (ratio  of  side  to  depth  length).    It  would, 
however,  for  this  frequency  analysis,  appear  that  the  element  formulations  available  to 
address  poor  aspect  ratios  (elform=-1  or  -2)  do  not  offer  much  improvement.    The 
constant stress solid (elform=1), the fully integrated S/R solid (elform=2), and the fully 
integrated  quadratic  8  node  element  with  nodal  rotations  (elform=3)  formulation  all 
appear to provide more than adequate results for this frequency study. 
The fully integrated S/R solid (the efficient formulation choice) intended to address poor 
aspect ratios (elform=-1), provided somewhat different shapes for modes 9 and 10.  This
stiffness reduction for certain modes (according to Borrvall [2009]).  However, modes 9 
and 10 are not those modes Borrvall offered concerns for in stiffness reduction. 
Eigenvalue Results: 
From  the  eigout  file,  generated  by  the  *CONTROL_IMPLICIT_EIGENVALUE 
keyword: 
Constant stress solid (elform=1): 
Simply Supported Square Plate: Out-of-Plane Vibration                    
r e s u l t s   o f   e i g e n v a l u e   a n a l y s i s: 
                             |------ frequency -----| 
        MODE    EIGENVALUE       RADIANS        CYCLES        PERIOD 
           1  -3.201421E-10   1.789252E-05   2.847682E-06   3.511628E+05 
           2   1.062290E-09   3.259279E-05   5.187303E-06   1.927784E+05 
           3   2.881279E-09   5.367755E-05   8.543047E-06   1.170543E+05 
           4   7.657028E+04   2.767133E+02   4.404030E+01   2.270648E-02 
           5   4.475080E+05   6.689604E+02   1.064684E+02   9.392462E-03 
           6   4.475080E+05   6.689604E+02   1.064684E+02   9.392462E-03 
           7   9.548827E+05   9.771810E+02   1.555232E+02   6.429910E-03 
           8   1.479411E+06   1.216310E+03   1.935818E+02   5.165775E-03 
           9   1.581263E+06   1.257483E+03   2.001346E+02   4.996637E-03 
          10   1.581263E+06   1.257483E+03   2.001346E+02   4.996637E-03 
Fully integrated S/R solid (elform=2) 
Simply Supported Square Plate: Out-of-Plane Vibration                    
r e s u l t s   o f   e i g e n v a l u e   a n a l y s i s: 
                             |------ frequency -----| 
        MODE    EIGENVALUE       RADIANS        CYCLES        PERIOD 
           1  -6.009941E-09   7.752381E-05   1.233830E-05   8.104846E+04 
           2   9.895302E-10   3.145680E-05   5.006505E-06   1.997401E+05 
           3   5.558832E-09   7.455757E-05   1.186621E-05   8.427293E+04 
           4   9.289190E+04   3.047817E+02   4.850752E+01   2.061536E-02 
           5   5.721748E+05   7.564224E+02   1.203884E+02   8.306451E-03 
           6   5.721748E+05   7.564224E+02   1.203884E+02   8.306451E-03 
           7   1.135577E+06   1.065635E+03   1.696010E+02   5.896191E-03 
           8   1.478563E+06   1.215962E+03   1.935263E+02   5.167257E-03 
           9   1.582107E+06   1.257818E+03   2.001880E+02   4.995304E-03 
          10   1.582107E+06   1.257818E+03   2.001880E+02   4.995304E-03 
Fully integrated S/R solid - for poor aspect ratio (eff) - (elform=-1) 
Simply Supported Square Plate: Out-of-Plane Vibration                    
r e s u l t s   o f   e i g e n v a l u e   a n a l y s i s: 
                             |------ frequency -----| 
        MODE    EIGENVALUE       RADIANS        CYCLES        PERIOD 
           1   1.043372E-08   1.021456E-04   1.625698E-05   6.151205E+04 
           2   1.335866E-08   1.155797E-04   1.839507E-05   5.436238E+04 
           3   1.573062E-08   1.254218E-04   1.996149E-05   5.009645E+04 
           4   8.154482E+04   2.855605E+02   4.544837E+01   2.200299E-02 
           5   4.529502E+05   6.730158E+02   1.071138E+02   9.335866E-03 
           6   4.529502E+05   6.730158E+02   1.071138E+02   9.335866E-03 
           7   9.993359E+05   9.996679E+02   1.591021E+02   6.285273E-03 
           8   1.478432E+06   1.215908E+03   1.935178E+02   5.167484E-03 
           9   1.560100E+06   1.249040E+03   1.987908E+02   5.030413E-03
Fully integrated S/R solid - for poor aspect ratio (acc) - (elform=-2) 
Simply Supported Square Plate: Out-of-Plane Vibration                    
r e s u l t s   o f   e i g e n v a l u e   a n a l y s i s: 
                             |------ frequency -----| 
        MODE    EIGENVALUE       RADIANS        CYCLES        PERIOD 
           1   2.211891E-09   4.703075E-05   7.485176E-06   1.335974E+05 
           2   7.014023E-09   8.374977E-05   1.332919E-05   7.502332E+04 
           3   1.121953E-08   1.059223E-04   1.685805E-05   5.931883E+04 
           4   8.428602E+04   2.903205E+02   4.620595E+01   2.164223E-02 
           5   4.713255E+05   6.865315E+02   1.092649E+02   9.152072E-03 
           6   4.713255E+05   6.865315E+02   1.092649E+02   9.152072E-03 
           7   1.061078E+06   1.030087E+03   1.639434E+02   6.099667E-03 
           8   1.478558E+06   1.215960E+03   1.935260E+02   5.167264E-03 
           9   1.581923E+06   1.257745E+03   2.001764E+02   4.995595E-03 
          10   1.581923E+06   1.257745E+03   2.001764E+02   4.995595E-03 
Fully integrated quadratic 8 node element with nodal rotations (elform=3) 
Simply Supported Square Plate                                            
r e s u l t s   o f   e i g e n v a l u e   a n a l y s i s: 
                             |------ frequency -----| 
        MODE    EIGENVALUE       RADIANS        CYCLES        PERIOD 
           1   1.877197E-08   1.370108E-04   2.180595E-05   4.585904E+04 
           2   2.239540E-08   1.496509E-04   2.381768E-05   4.198561E+04 
           3   2.614979E-08   1.617090E-04   2.573678E-05   3.885490E+04 
           4   7.425572E+04   2.724990E+02   4.336957E+01   2.305764E-02 
           5   4.327897E+05   6.578675E+02   1.047029E+02   9.550837E-03 
           6   4.327897E+05   6.578675E+02   1.047029E+02   9.550837E-03 
           7   9.345968E+05   9.667455E+02   1.538623E+02   6.499317E-03 
           8   1.473997E+06   1.214083E+03   1.932273E+02   5.175253E-03 
           9   1.524111E+06   1.234549E+03   1.964846E+02   5.089458E-03 
          10   1.536475E+06   1.239546E+03   1.972799E+02   5.068940E-03 
Mode Shapes: 
The  constant  stress  solid  (elform=1)  mode  shapes  are  shown  in  Figure  12.2,  the  fully 
integrated  S/R  solid  (elform=2)  in  Figure  12.3,  the  fully  integrated  quadratic  8  node 
element with nodal rotations (elform=3) in Figure 12.4, the fully integrated S/R solid (the 
so-called efficient formulation choice) intended to address poor aspect ratios (elform=-1) 
in  Figure  12.5,  and  the  fully  integrated  S/R  solid  (the  so-called  accurate  formulation 
choice) intended to address poor aspect ratios (elform=-2) in Figure 12.6. 
The first three modes are not shown (rigid body translations).  Modes 4 through 10 are 
shown for the selected results.  Modes 5 and 6 are identical for all element formulations; 
modes  9  and  10  are  also  identical  for  all,  with  the  exception  of  the  fully  integrated
Figure 12.2 - Mode shapes for constant stress solid (elform=1).
Figure 12.4 - Mode shapes for fully integrated quadratic 8 node 
element with nodal rotations (elform=3).
Figure 12.6 - Mode shapes fully integrated S/R solid (elform=-2). 
Input deck: 
*KEYWORD 
*TITLE 
Simply Supported Square Plate: Out-of-Plane Vibration (solid mesh) 
*CONTROL_IMPLICIT_EIGENVALUE 
$#    neig    center     lflag    lftend     rflag    rhtend    eigmth    shfscl 
        10       0.0         0       0.0         0       0.0         0       0.0 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form 
         1       0.0 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
  1.000000         0       0.0       0.0       0.0 
*DATABASE_BINARY_D3PLOT 
$# dt/cycl   lcdt/nr      beam     npltc    psetid 
  1.000000 
*ELEMENT_SOLID 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       1      37      41       5       2      38      42       6 
     192       1     283     319     323     287     284     320     324     288 
*NODE 
$#   nid               x               y               z      tc      rc 
       1             0.0             0.0             0.0       3 
     324     10.00000000     10.00000000      1.00000000 
*BOUNDARY_SPC_SET 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         1         0         0         0         1 
*PART 
$# title                                                                         
material type # 1  (Elastic)
$#   secid    elform       aet 
         1         1         1 
$         1         2         1 
$         1        -1         1 
$         1        -2         1 
$         1         3         1 
*MAT_ELASTIC 
$#     mid        ro         e        pr        da        db  not used 
         1  8000.0002.0000e+11  0.300000       0.0       0.0       0.0 
*HOURGLASS 
$#    hgid       ihq        qm       ibq        q1        q2        qb        qw 
         1         6       1.0         0       0.0       0.0       0.0       0.0 
*SET_NODE_LIST 
$#     sid       da1       da2       da3       da4    solver 
         1       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         1        37        73       109       145       181       217       253 
       289       293       297       301       305       309       313       317 
       321       285       249       213       177       141       105        69 
        33        29        25        21        17        13         9         5 
*END
13.  Simply Supported Square Plate: Out-of-Plane Vibration 
(thick shell mesh) 
Keywords: 
*CONTROL_IMPLICIT_EIGENVALUE 
*CONTROL_IMPLICIT_GENERAL 
Description: 
Determine the first 10 natural frequencies of a solid simply-supported plate of thickness 
t=1.0  m.    Each  side  of  the  plate  measure  10.0  m.    The  plate  is  meshed  with  solid 
hexahedra  element  with  an  8  x  8  x  3  density.    On  the  lower  surface,  outer  boundary 
nodes, 
ZU = . 
The finite element model is shown in Figure 13.1. 
Figure 13.1 – Finite element model with simply supported
Analysis Summary: 
Dim.  Type  Load  Material  Geometry  Contact 
Solver 
3D  Modal 
- 
Linear 
Linear 
- 
Implicit 
Solution 
Method 
Block Shift 
and Inverted 
Lanczos 
Units: 
kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) 
Dimensional Data: 
Rectangular dimensions of square plate: 10.0 m x 10.0 m x 1.00 m. 
Material Data: 
Mass Density 
Young's Modulus 
Poisson's Ratio 
ρ=
=
ν =
Element Types: 
11
×
8.00 10
×
2.00 10
0.3
/kg m
Pa
S/R 2x2 IPI thick shell (elform=2) 
Assumed strain 2x2 IPI thick shell (elform=3) 
Assumed strain RI thick shell (elform=5) 
Material Models: 
*MAT_001 or *MAT_ELASTIC 
Results Comparison: 
LS-DYNA natural frequencies, first 10 (frequency in Hertz), and mode shapes (4 through
Mode(s) 
NAFEMS 
FV52 (Hz) 
elform=2 (Hz) 
elform=3 (Hz) 
elform=5 (Hz) 
1, 2, 3 
rigid body 
rigid body 
rigid body 
rigid body 
4 
45.897 
43.480 
42.556 
44.656 
5, 6 
109.440 
105.363 
102.983 
107.290 
7 
8 
9 
167.890 
152.764 
150.187 
157.397 
193.590 
185.301 
193.378 
193.583 
206.190 
193.708 
197.247 
200.136 
10 
206.190 
200.997 
197.295 
200.136 
The assumed strain 2x2 IPI thick shell (elform=3) and the assumed strain RI thick shell 
(elform=5)  use  a  full  three-dimensional  stress  update  rather  than  the  two-dimensional 
plane  stress  update  of  the  one  point  reduced  integration  (elform=1)  and  the  selectively 
reduced 2x2 IPI thick shell (elform=2). 
The selectively reduced 2x2 IPI thick shell (elform=2), the assumed strain 2x2 IPI thick 
shell  (elform=3),  and  the  assumed  strain  RI  thick  shell  (elform=5)  all  provide  similar 
frequency results for this analysis. 
The  selectively  reduced  2x2  IPI  thick  shell  (elform=2)  formulation  appears  to  have 
identified (added)  an unexpected  result  for mode  8 (an  anomaly,  a  low energy warping 
mode which is believed will not cause solution troubles) due to the calculation of the out-
of-plane  shear  stiffness  terms.    Code  inspection  indicated  that  the  out-of-plane  shear 
stress and stiffness is calculated at the mid-point rather than the 2x2 integration points in 
order  to  prevent  shear  locking  in  bending.    Modes  9  and  10  (elform=2)  are  however, 
similar to modes 8 and 9, respectively, for the assumed strain RI thick shell (elform=5) 
formulation. 
The assumed strain 2x2 IPI thick shell (elform=3) formulation appears to have identified 
two  different  modes  and  frequencies  for  modes  9  and  10.    This  is  possibly  due  to  the 
employment of a corotational system that rotates with the elements, which suppresses the
Eigenvalue Results: 
From  the  eigout  file,  generated  by  the  *CONTROL_IMPLICIT_EIGENVALUE 
keyword: 
S/R 2x2 IPI thick shell (elform=2) 
Simply Supported Square Plate: Out-of-Plane Vibration (thick shell mesh) 
r e s u l t s   o f   e i g e n v a l u e   a n a l y s i s: 
                             |------ frequency -----| 
        MODE    EIGENVALUE       RADIANS        CYCLES        PERIOD 
           1  -8.469215E-09   9.202834E-05   1.464676E-05   6.827446E+04 
           2  -3.463356E-09   5.885028E-05   9.366313E-06   1.067656E+05 
           3  -1.746230E-09   4.178791E-05   6.650753E-06   1.503589E+05 
           4   7.449258E+04   2.729333E+02   4.343868E+01   2.302096E-02 
           5   4.377512E+05   6.616277E+02   1.053013E+02   9.496558E-03 
           6   4.377512E+05   6.616277E+02   1.053013E+02   9.496558E-03 
           7   9.193747E+05   9.588403E+02   1.526042E+02   6.552901E-03 
           8   1.255008E+06   1.120271E+03   1.782967E+02   5.608628E-03 
           9   1.481334E+06   1.217101E+03   1.937076E+02   5.162420E-03 
          10   1.594925E+06   1.262903E+03   2.009973E+02   4.975191E-03 
Assumed strain 2x2 IPI thick shell (elform=3) 
Simply Supported Square Plate: Out-of-Plane Vibration (thick shell mesh) 
r e s u l t s   o f   e i g e n v a l u e   a n a l y s i s: 
                             |------ frequency -----| 
        MODE    EIGENVALUE       RADIANS        CYCLES        PERIOD 
           1  -8.338247E-09   9.131400E-05   1.453308E-05   6.880856E+04 
           2  -4.802132E-09   6.929742E-05   1.102903E-05   9.066983E+04 
           3  -3.012246E-09   5.488394E-05   8.735050E-06   1.144813E+05 
           4   7.149598E+04   2.673873E+02   4.255601E+01   2.349844E-02 
           5   4.186854E+05   6.470590E+02   1.029826E+02   9.710374E-03 
           6   4.186854E+05   6.470590E+02   1.029826E+02   9.710374E-03 
           7   8.904817E+05   9.436534E+02   1.501871E+02   6.658361E-03 
           8   1.476299E+06   1.215030E+03   1.933781E+02   5.171217E-03 
           9   1.535967E+06   1.239341E+03   1.972473E+02   5.069778E-03 
          10   1.536702E+06   1.239638E+03   1.972945E+02   5.068565E-03 
Assumed strain RI thick shell (elform=5) 
Simply Supported Square Plate: Out-of-Plane Vibration (thick shell mesh) 
r e s u l t s   o f   e i g e n v a l u e   a n a l y s i s: 
                             |------ frequency -----| 
        MODE    EIGENVALUE       RADIANS        CYCLES        PERIOD 
           1   5.966285E-10   2.442598E-05   3.887516E-06   2.572337E+05 
           2   2.881279E-09   5.367755E-05   8.543047E-06   1.170543E+05 
           3   5.762558E-09   7.591152E-05   1.208169E-05   8.276986E+04 
           4   7.872674E+04   2.805829E+02   4.465615E+01   2.239333E-02 
           5   4.544420E+05   6.741231E+02   1.072900E+02   9.320531E-03 
           6   4.544420E+05   6.741231E+02   1.072900E+02   9.320531E-03 
           7   9.780258E+05   9.889519E+02   1.573966E+02   6.353378E-03 
           8   1.479432E+06   1.216319E+03   1.935832E+02   5.165738E-03 
           9   1.581277E+06   1.257488E+03   2.001355E+02   4.996615E-03
Mode Shapes: 
The first three modes are not shown (rigid body translations).  Modes 4 through 10 are 
shown for the selected results.  Modes 5 and 6 are identical for all element formulations.  
Modes 9 and 10 offer three different sets of results, depending on  element formulation; 
(1) for selectively reduced 2x2 IPI thick shell (elform=2), there is a distinct difference in 
natural frequencies (Figure 13.2), (2) for assumed strain 2x2 IPI thick shell (elform=3), 
there is a  very slight difference (Figure  13.3), and (3) for assumed  strain RI thick shell 
(elform=5), the results are identical (Figure 13.4).
Figure 13.3 - Mode shapes for assumed strain 2x2 IPI thick shell (elform=3).
*TITLE 
Simply Supported Square Plate: Out-of-Plane Vibration (thick shell mesh) 
*CONTROL_IMPLICIT_EIGENVALUE 
$#    neig    center     lflag    lftend     rflag    rhtend    eigmth    shfscl 
        10       0.0         0       0.0         0       0.0         0       0.0 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form 
         1       0.0 
*CONTROL_SHELL 
$#  wrpang     esort     irnxx    istupd    theory       bwc     miter      proj 
  20.00000         0         0         0         2         2         1 
$# rotascl    intgrd    lamsht    cstyp6    tshell    nfail1    nfail4 
       0.0         1 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
  1.000000         0       0.0       0.0       0.0 
*DATABASE_BINARY_D3PLOT 
$# dt/cycl   lcdt/nr      beam     npltc    psetid 
  1.000000 
*ELEMENT_TSHELL 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       1      37      41       5       2      38      42       6 
     192       1     283     319     323     287     284     320     324     288 
*NODE 
$#   nid               x               y               z      tc      rc 
       1             0.0             0.0             0.0       3 
     324     10.00000000     10.00000000      1.00000000 
*BOUNDARY_SPC_SET 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         1         0         0         0         1 
*PART 
$# title                                                                         
material type # 1  (Elastic)                                                     
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1         0         1 
*SECTION_TSHELL 
$#   secid    elform      shrf       nip     propt   qr/irid     icomp    tshear 
         1         2       0.0         5         0       0.0 
$         1         3       0.0         5         0       0.0 
$         1         5       0.0         5         0       0.0 
*MAT_ELASTIC 
$#     mid        ro         e        pr        da        db  not used 
         1  8000.0002.0000e+11  0.300000       0.0       0.0       0.0 
*HOURGLASS 
$#    hgid       ihq        qm       ibq        q1        q2        qb        qw 
         1         4       0.1         0       0.0       0.0       0.0       0.0 
*SET_NODE_LIST 
$#     sid       da1       da2       da3       da4    solver 
         1       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         1        37        73       109       145       181       217       253 
       289       293       297       301       305       309       313       317 
       321       285       249       213       177       141       105        69 
        33        29        25        21        17        13         9         5 
*END 
Notes: 
1.  The  assumed  strain  2x2  IPI  thick  shell  (elform=3)  and  the  assumed  strain  RI  thick 
shell  (elform=5)  are  distortion  sensitive  and  should  not  be  used  in  situations  where
2.  With the one point reduced integration (elform=1) and the selectively reduced 2x2 IPI 
thick  shell  (elform=2),  a  single  element  through  the  thickness  will  capture  bending 
response, but with the assumed strain 2x2 IPI thick shell (elform=3) and the assumed 
strain  RI  thick  shell  (elform=5),  two  elements  are  recommended  to  avoid  excessive 
softness. 
3.  Only the selectively  reduced 2x2  IPI thick shell (elform=2), the assumed strain 2x2 
IPI  thick  shell  (elform=3),  and  the  assumed  strain  RI  thick  shell  (elform=5)  are 
available  for  implicit  applications.    If  one  point  reduced  integration  (elform=1)  is 
specified in an  implicit  analysis,  it is  internally  switched to selectively  reduced 2x2
14.  Simply Supported Square Plate: Transient Forced 
Vibration (solid mesh) 
Keywords: 
*CONTROL_IMPLICIT_AUTO 
*CONTROL_IMPLICIT_DYNAMICS 
*CONTROL_IMPLICIT_GENERAL 
*CONTROL_IMPLICIT_SOLVER 
*CONTROL_IMPLICIT_SOLUTION 
Description: 
A  plate  is  subjected  to  a  suddenly  applied  pressure  on  its  top.    A  transient  analysis  is 
performed in order to obtain the response of the plate.  Damping is present.  On the lower 
surface, outer boundary nodes, 
ZU = . 
The finite element model is shown in Figure 14.1. 
Figure 14.1 – Finite element model with applied pressure on upper surface and
Analysis Summary: 
Dim. 
Type 
Load  Material  Geometry  Contact 
Solver 
Solution 
Method 
3D  Dynamic 
Pressure 
Damping 
Linear 
Linear 
- 
Implicit 
1 - Linear 
Units: 
kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) 
Dimensional Data: 
Rectangular dimensions of square plate: 10.0 m x 10.0 m x 1.00 m. 
Material Data: 
Mass Density 
Young's Modulus 
Poisson's Ratio 
Damping ratio 
Load: 
Pressure 
Element Types: 
/kg m
Pa
11
ρ=
×
8.00 10
×
=
2.00 10
ν =
0.3
%2=ζ
=
×
1.0 10
Pa
Constant stress solid (elform=1) 
Fully integrated S/R solid (elform=2) 
Fully integrated S/R solid - for poor aspect ratio (eff) - (elform=-1) 
Fully integrated S/R solid - for poor aspect ratio (acc) - (elform=-2) 
Fully integrated quadratic 8 node element with nodal rotations (elform=3) 
Material Models: 
*MAT_001 or *MAT_ELASTIC 
Damping:
id
ωζ2=
As the excited mode is the first, corresponding to 
) 
(that from  NAFEMS Benchmark Test  FV52),  we  choose the  damping  factor relative  to 
the first frequency: 
288.380
45.897
rad s
Hz
 (
/
ω =
=
1 11.535
=
Hz
Results Comparison: 
LS-DYNA X-direction bending stress, σxx , at (Node 161) on bottom surface plus its Z-
displacement,
ZU ,  are  compared  with  NAFEMS  Selected  Benchmarks  for  Forced 
Vibration, Test 21T. 
Reference Condition - Center 
(Node 161) 
Peak Bending 
Stress σxx  (Pa) 
Peak 
ZU (m) 
Steady-State 
ZU (m) 
NAFEMS Benchmark Test 21T 
6.211 10×
4.524 10−
×
−
2.333 10−
×
−
Constant stress solid (elform=1) 
4.638 10×
5.438 10−
×
−
2.778 10−
×
−
Fully integrated S/R solid 
(elform=2) 
Fully integrated S/R solid 
(elform=-1) 
Fully integrated S/R solid 
(elform=-2) 
3.732 10×
3.925 10−
×
−
2.019 10−
×
−
4.611 10×
4.435 10−
×
−
2.242 10−
×
−
4.221 10×
4.365 10−
×
−
2.203 10−
×
−
Fully integrated quadratic element 
with nodal rotations (elform=3) 
x xxx ×
.
10
−
x xxx
.
×
10
−
−
x xxx
.
×
10
−
The constant stress solid (elform=1) result of
×
4.638 10 Pa
 is an element centroid value. 
These nodal displacement results were generated by *DATABASE_NODOUT keyword 
while  the  axial  stress  (nodal)  results  were  generated  by  *DATABASE_ELOUT  (elout 
file)  and  *DATABASE_EXTENT_BINARY  (eloutdet  file  provides  detailed  element 
output at integration points and connectivity nodes) keyword entries. 
You  can  set  intout=stress  or  intout=all  (*DATABASE_EXTENT_BINARY)  and  have 
file  called  eloutdet 
integration  points 
stresses  output 
for  all 
to  a
(*DATABASE_ELOUT  governs  the  output  interval  and  *DATABASE_HISTORY_ 
SOLID  governs  which  elements  are  output).    Setting  nodout=stress  or  nodout=all  in 
*DATABASE_EXTENT_BINARY will write the extrapolated nodal stresses to eloutdet. 
LS-DYNA stress and strain output corresponds to integration point locations.  Stress at a 
node  is  an  artifact  of  the  post-processor  and  represents  an  average  of  the  surrounding 
integration  point  stresses  (the  value  will  likely  be  different  with  different  post-
processors). 
For  this  coarse  mesh,  the  one-point  quadrature  (low  order)  constant  stress  solid 
(elform=1) element  formulation (the  LS-DYNA default) provides a less stiff, stress and 
displacement comparison.  Refinement of the mesh should provide a better comparison. 
The  higher  order,  fully  integrated  selectively  reduced  solid  (elform=2)  provides  a 
comparatively  stiff  result,  both  in  stress  and  displacement,  probably  due  to  the  coarse 
mesh. 
The  aspect  ratio  of  these  elements  is  3.75  (ratio  of  side  to  depth  length).    Available 
options  are  the  higher  order,  fully  integrated  S/R  solid  (both  the  so-called  efficient  and 
the  so-called  accurate  formulation  choices)  intended  to  address  poor  aspect  ratios 
(elform=-1  and  -2,  respectively).    These  formulations  provide  a  good  comparison  of 
displacements  (peak  and  steady-state)  for  this  coarse  mesh.    Unfortunately,  the  stress 
comparison is not very good; it is not understood why at this time. 
The  fully  integrated  S/R  solid  (the  so-called  efficient  formulation  choice)  intended  to 
address poor aspect ratios (elform=-1), can provide a slightly less stiff solution than the 
so-called accurate formulation choice (elform=2).  This formulation (elform=-1) involves 
a  slight  modification  of  the  Jacobian  matrix  which  can  lead  to  a  stiffness  reduction  for 
certain  modes,  in  particular  the  out-of-plane  hourglass  mode  (according  to  Borrvall 
[2009]). 
The  higher  order,  fully  integrated  quadratic  8  node  element  with  nodal  rotations 
(elform=3) formulation provides a (????) results.  Waiting for LSTC LS-DYNA code fix 
to remark on this. 
For  the  fully  integrated  S/R  solid  accurate  formulation  (elform=-2),  the  contour  plot  of 
the X-direction bending  stress  (Figure 14.2) and  the Z-displacement (Figure 14.3) were 
obtained  from  the  d3plot  file  at  peak  displacement  time  which  were  generated  by  the
Figure 14.2 – Contour plot of the X-stress (elform=-2) at peak displacement time.
*TITLE 
Simply Supported Square Plate: Transient Forced Vibration (solid mesh) 
*CONTROL_IMPLICIT_AUTO 
$#   iauto    iteopt    itewin     dtmin     dtmax     dtexp     kfail    kcycle 
         0        11         5       0.0       0.0 
*CONTROL_IMPLICIT_DYNAMICS 
$#   imass     gamma      beta 
         1  0.500000  0.250000 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form    zero_v 
         1  0.000100         2         1         2 
*CONTROL_IMPLICIT_SOLVER 
$#  lsolvr    lprint     negev     order      drcm    drcprm   autospc   autotol 
         4         2         2         0         1       0.0         1       0.0 
$#  lcpack 
         2 
*CONTROL_IMPLICIT_SOLUTION 
$#  nsolvr    ilimit    maxref     dctol     ectol     rctol     lstol    abstol 
         2        11        15    0.0010    0.0100  1.00e+10  0.900000  1.000000 
$#   dnorm    diverg     istif   nlprint 
         2         1         1         2 
$#  arcctl    arcdir    arclen    arcmth    arcdmp 
         0         1       0.0         1         2 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
  0.020000         0       0.0       0.0       0.0 
*DATABASE_ELOUT 
$#      dt    binary      lcur     ioopt 
1.0000e-06         1 
*DATABASE_NODFOR 
$#      dt    binary      lcur     ioopt 
1.0000e-06         1 
*DATABASE_NODOUT 
$#      dt    binary      lcur     ioopt 
1.0000e-06         1 
*DATABASE_BINARY_D3PLOT 
$# dt/cycl 
  0.001000 
*DATABASE_EXTENT_BINARY 
$#   neiph     neips    maxint    strflg    sigflg    epsflg     rtflg    engflg 
$#  cmpflg    ieverp    beamip     dcomp      shge     stssz    n3thdt   ialemat 
$# nintsld   pkp_sen      sclp     hydro     msscl     therm    intout    nodout 
         8                 1.0                                  stress    stress 
*DATABASE_HISTORY_SOLID 
$#     id1       id2       id3       id4       id5       id6       id7       id8 
        28        29        36        37 
*DATABASE_NODAL_FORCE_GROUP 
$#    nsid       cid 
       164 
*DATABASE_HISTORY_NODE 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
       161       164 
*SET_NODE_LIST 
$#     sid       da1       da2       da3       da4    solver 
       164       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
       164 
*DAMPING_GLOBAL 
$#    lcid    valdmp       stx       sty       stz       srx       sry       srz 
         0  11.53500       0.0       0.0       0.0       0.0       0.0       0.0 
*DEFINE_CURVE 
$#    lcid      sdir       sfa       sfo      offa      offo     dattyp 
         1         0       0.0       0.0       0.0       0.0 
$#                a1                  o1
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       1      37      41       5       2      38      42       6 
     192       1     283     319     323     287     284     320     324     288 
*NODE 
$#   nid               x               y               z      tc      rc 
       1             0.0             0.0             0.0       3 
     324     10.00000000     10.00000000      1.00000000 
*BOUNDARY_SPC_SET 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         1         0         0         0         1 
*PART 
$# title                                                                         
material type # 1  (Elastic)                                                     
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1 
*SECTION_SOLID 
$#   secid    elform       aet 
         1         1         1 
$         1         2         1 
$         1        -1         1 
$         1        -2         1 
$         1         3         1 
*MAT_ELASTIC 
$#     mid        ro         e        pr        da        db  not used 
         1  8000.0002.0000e+11  0.300000       0.0       0.0       0.0 
*LOAD_SEGMENT 
$#    lcid        sf        at        n1        n2        n3        n4 
         1  1.000000       0.0         4        40        44         8 
         1  1.000000       0.0       284       320       324       288 
*SET_NODE_LIST 
$#     sid       da1       da2       da3       da4    solver 
         1       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         1        37        73       109       145       181       217       253 
       289       293       297       301       305       309       313       317 
       321       285       249       213       177       141       105        69 
        33        29        25        21        17        13         9         5 
*END 
Notes: 
1.  One  should  remember  that  the  constant  stress  solid  (elform=1),  the  fully  integrated 
S/R solid (elform=2), and the fully integrated S/R solid (both the so-called efficient 
and the so-called accurate formulation choices) intended to address poor aspect ratios 
(elform=-1  and  -2,  respectively)  were  originally  developed  for  performing  highly
15.  Simply Supported Square Plate: Transient Forced 
Vibration (thick shell mesh) 
Keywords: 
*CONTROL_IMPLICIT_AUTO 
*CONTROL_IMPLICIT_DYNAMICS 
*CONTROL_IMPLICIT_GENERAL 
*CONTROL_IMPLICIT_SOLVER 
*CONTROL_IMPLICIT_SOLUTION 
Description: 
A  plate  is  subjected  to  a  suddenly  applied  pressure  on  its  top.    A  transient  analysis  is 
performed in order to obtain the response of the plate.  Damping is present.  On the lower 
surface, outer boundary nodes, 
ZU = . 
The finite element model is shown in Figure 15.1. 
Figure 15.1 – Finite element model with applied pressure on upper surface and
Analysis Summary: 
Dim. 
Type 
Load  Material  Geometry  Contact 
Solver 
Solution 
Method 
3D  Dynamic 
Pressure 
Damping 
Linear 
Linear 
- 
Implicit 
1 - Linear 
Units: 
kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) 
Dimensional Data: 
Rectangular dimensions of square plate: 10.0 m x 10.0 m x 1.00 m. 
Material Data: 
Mass Density 
Young's Modulus 
Poisson's Ratio 
Damping ratio 
Load: 
Pressure 
Element Types: 
/kg m
Pa
11
ρ=
×
8.00 10
=
×
2.00 10
ν =
0.3
%2=ζ
=
×
1.0 10
Pa
S/R 2x2 IPI thick shell (elform=2) 
Assumed strain 2x2 IPI thick shell (elform=3) 
Assumed strain RI thick shell (elform=5) 
Material Models: 
*MAT_001 or *MAT_ELASTIC 
Damping: 
The damping factor  d  is easily found from the natural frequency of the system: 
id
ωζ2=
) 
As the excited mode is the first, corresponding to 
(that from NAFEMS  Benchmark Test  FV52),  we  choose the  damping  factor relative  to 
the first frequency: 
288.380
45.897
rad s
Hz
 (
/
ω =
=
1 11.535
=
Hz
Results Comparison: 
LS-DYNA X-direction bending stress, σxx , at (Node 161) on bottom surface plus its Z-
displacement,
ZU ,  are  compared  with  NAFEMS  Selected  Benchmarks  for  Forced 
Vibration, Test 21T. 
Reference Condition - Center 
(Node 161) 
Peak Bending 
Stress σxx  (Pa) 
Peak 
ZU (m) 
Steady-State 
ZU (m) 
NAFEMS Benchmark Test 21T 
6.211 10×
4.524 10−
×
−
2.333 10−
×
−
S/R 2x2 IPI thick shell (elform=2) 
6.398 10×
4.937 10−
×
−
2.537 10−
×
−
Assumed strain 2x2 IPI thick shell 
(elform=3) 
Assumed strain RI thick shell 
(elform=5) 
6.350 10×
5.090 10−
×
−
2.616 10−
×
−
6.319 10×
5.022 10−
×
−
2.557 10−
×
−
These nodal displacement results were generated by *DATABASE_NODOUT keyword 
while  the  axial  stress  (nodal)  results  were  generated  by  *DATABASE_ELOUT  (elout 
file)  and  *DATABASE_EXTENT_BINARY  (eloutdet  file  provides  detailed  element 
output at integration points and connectivity nodes) keyword entries. 
You  can  set  intout=stress  or  intout=all  (*DATABASE_EXTENT_BINARY)  and  have 
stresses  output 
file  called  eloutdet 
integration  points 
(*DATABASE_ELOUT  governs  the  output  interval  and  *DATABASE_HISTORY_ 
TSHELL  governs  which  elements  are  output).    Setting  nodout=stress  or  nodout=all  in 
*DATABASE_EXTENT_BINARY will write the extrapolated nodal stresses to eloutdet. 
for  all 
to  a 
the 
LS-DYNA stress and strain output corresponds to integration point locations.  Stress at a 
node  is  an  artifact  of  the  post-processor  and  represents  an  average  of  the  surrounding 
integration  point  stresses  (the  value  will  likely  be  different  with  different  post-
Lobatto  integration  (intgrd=1  -  *CONTROL_SHELL)  was  employed  since  it  has  an 
advantage in that the inner and outer integration points are on the shell surfaces.  Gauss 
integration  is  the  default  through  thickness  integration  rule  (the  default  number  of 
through  thickness  integration  points  is  nip=2  -  *SECTION_TSHELL)  in  LS-DYNA, 
where 1-10 integration points may be specified, whereas, with Lobatto integration, 3-10 
integration  points  may  be  specified  (for  2  point  integration,  the  Lobatto  rule  is  very 
inaccurate). 
The selectively reduced 2x2 IPI thick shell (elform=2), the assumed strain 2x2 IPI thick 
shell  (elform=3),  and  the  assumed  strain  RI  thick  shell  (elform=5)  all  provide  similar 
results  for  this  transient  forced  vibration  example,  though  slightly  less  stiff  in 
comparison, both in stress and displacement. 
Remember  that  (a)  only  the  higher  order,  selectively  reduced  2x2  IPI  thick  shell 
(elform=2)  provides  a  reasonable  stress  comparison  for  a  single  element  through  the 
thickness,  although  with  a  comparatively  stiff  result,  and  (b)  the  higher  order,  assumed 
strain  2x2  IPI  thick  shell  (elform=3)  and  assumed  strain  RI  thick  shell  (elform=5) 
formulations  do  provide  acceptable  results  with  at  least  two  elements  through  the 
thickness (recommended) to capture the bending response. 
For this transient forced vibration example, with an element aspect ratio of 3.75, it is seen 
that  the  thick  shell  formulations,  on  the  whole,  compare  better  than  the  solid  element 
formulation  results.    The  exception  to  this  would  be  the  displacement  comparison 
provided  by  the  higher  order,  fully  integrated  S/R  solid  (both  so-called  efficient  and 
accurate  formulation  choices)  intended  to  address  poor  aspect  ratios  (elform=-1  and  -2, 
respectively). 
For  the  selectively  reduced  2x2  IPI  thick  shell  (elform=2),  the  contour  plot  of  the  X-
direction  bending  stress  (Figure  15.2)  and  the  Z-displacement  (Figure  15.3)  were 
obtained  from  the  d3plot  file  at  peak  displacement  time  which  were  generated  by  the
Figure 15.2 – Contour plot of the X-stress (elform=2) at peak displacement time.
*TITLE 
Simply Supported Square Plate: Transient Forced Vibration (thick shell mesh) 
*CONTROL_IMPLICIT_AUTO 
$#   iauto    iteopt    itewin     dtmin     dtmax     dtexp     kfail    kcycle 
         0        11         5       0.0       0.0 
*CONTROL_IMPLICIT_DYNAMICS 
$#   imass     gamma      beta 
         1  0.500000  0.250000 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form    zero_v 
         1  0.000100         2         1         2 
*CONTROL_IMPLICIT_SOLVER 
$#  lsolvr    lprint     negev     order      drcm    drcprm   autospc   autotol 
         4         2         2         0         1       0.0         1       0.0 
$#  lcpack 
         2 
*CONTROL_IMPLICIT_SOLUTION 
$#  nsolvr    ilimit    maxref     dctol     ectol     rctol     lstol    abstol 
         2        11        15    0.0010    0.0100  1.00e+10  0.900000  1.000000 
$#   dnorm    diverg     istif   nlprint 
         2         1         1         2 
$#  arcctl    arcdir    arclen    arcmth    arcdmp 
         0         1       0.0         1         2 
*CONTROL_SHELL 
$#  wrpang     esort     irnxx    istupd    theory       bwc     miter      proj 
  20.00000         0         0         0         2         2         1 
$# rotascl    intgrd    lamsht    cstyp6    tshell    nfail1    nfail4 
       0.0         1 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
  0.020000         0       0.0       0.0       0.0 
*DATABASE_ELOUT 
$#      dt    binary      lcur     ioopt 
1.0000e-06         1 
*DATABASE_NODFOR 
$#      dt    binary      lcur     ioopt 
1.0000e-06         1 
*DATABASE_NODOUT 
$#      dt    binary      lcur     ioopt 
1.0000e-06         1 
*DATABASE_BINARY_D3PLOT 
$# dt/cycl 
  0.001000 
*DATABASE_EXTENT_BINARY 
$#   neiph     neips    maxint    strflg    sigflg    epsflg     rtflg    engflg 
$#  cmpflg    ieverp    beamip     dcomp      shge     stssz    n3thdt   ialemat 
$# nintsld   pkp_sen      sclp     hydro     msscl     therm    intout    nodout 
         8                 1.0                                  stress    stress 
*DATABASE_HISTORY_TSHELL 
$#     id1       id2       id3       id4       id5       id6       id7       id8 
        28        29        36        37 
*DATABASE_NODAL_FORCE_GROUP 
$#    nsid       cid 
       164 
*DATABASE_HISTORY_NODE 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
       161       164 
*SET_NODE_LIST 
$#     sid       da1       da2       da3       da4    solver 
       164       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
       164 
*DAMPING_GLOBAL 
$#    lcid    valdmp       stx       sty       stz       srx       sry       srz
1         0       0.0       0.0       0.0       0.0 
$#                a1                  o1 
                 0.0       1.0000000e+06 
          0.10000000       1.0000000e+06 
*ELEMENT_TSHELL 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       1      37      41       5       2      38      42       6 
     192       1     283     319     323     287     284     320     324     288 
*NODE 
$#   nid               x               y               z      tc      rc 
       1             0.0             0.0             0.0       3 
     324     10.00000000     10.00000000      1.00000000 
*BOUNDARY_SPC_SET 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         1         0         0         0         1 
*PART 
$# title                                                                         
material type # 1  (Elastic)                                                     
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1 
*SECTION_TSHELL 
$#   secid    elform      shrf       nip     propt   qr/irid     icomp    tshear 
         1         2       0.0         5         0       0.0 
$         1         3       0.0         5         0       0.0 
$         1         5       0.0         5         0       0.0 
*MAT_ELASTIC 
$#     mid        ro         e        pr        da        db  not used 
         1  8000.0002.0000e+11  0.300000       0.0       0.0       0.0 
*LOAD_SEGMENT 
$#    lcid        sf        at        n1        n2        n3        n4 
         1  1.000000       0.0         4        40        44         8 
         1  1.000000       0.0       284       320       324       288 
*SET_NODE_LIST 
$#     sid       da1       da2       da3       da4    solver 
         1       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         1        37        73       109       145       181       217       253 
       289       293       297       301       305       309       313       317 
       321       285       249       213       177       141       105        69 
        33        29        25        21        17        13         9         5 
*END
16.  Transient Response of a Cylindrical Disk Impacting a 
Deformable Surface 
Keywords: 
*CONTROL_IMPLICIT_DYNAMICS 
*CONTROL_IMPLICIT_AUTO 
*CONTROL_IMPLICIT_GENERAL 
*CONTROL_IMPLICIT_SOLVER 
*CONTROL_IMPLICIT_SOLUTION 
*CONTACT_2D_AUTOMATIC_NODE_TO_SURFACE 
Description: 
A  rigid  cylindrical  disk  of  given  mass  (m)  is  released  from  1.0  inch  height  (h)  and, 
accelerated  by  gravity  (g),  hits  a  deformable  surface  of  given  stiffness  (k).    Plot  the 
velocity,  displacement, and kinetic energy  of  the disk,  plus identify the time of impact.  
The maximum displacement of the cylindrical disk is also to be determined. 
This  simulation  (Figure  16.1)  is  2D  plane  strain  (a  choice  of  the  available  LS-DYNA 
options to address the impact - with the objects being rigid, this can be seen to negate the 
need for any planar type definition).  The cylindrical disk is modeled with shell elements, 
x-y  plane,  which  do  not  need  additional  constraints  to  ensure  in-plane  behavior.    The 
deformable surface  is modeled  with rigid beam elements, x-y plane, to address contact, 
and  a  1D  translational  spring  element  of  a  finite  length  (l),  x-y  plane,  to  address  the 
deformation. 
As  a  geometric  convenience,  LS-DYNA  employs  the  *SECTION_SHELL  and 
*ELEMENT_SHELL entries to describe 2D plane stress, plane strain, and axisymmetric 
solids,  and  the  *SECTION_BEAM  and  *ELEMENT_BEAM  entries  to  describe  2D 
axisymmetric shells, and 2D plane strain beam elements. 
for 
suitable  contact  algorithm 
A 
the  *CONTACT_2D_ 
AUTOMATIC_NODE_TO_SURFACE.    For  this  algorithm,  the  contact  stiffness  is 
activated  when  a  node  nears  a  segment  at  some  given  tolerance.    The  stiffness  is 
increased as the node moves closer with the full stiffness being used when the nodal point 
finally makes contact.  Understanding LS-DYNA contact considerations adds to the focus 
of this example.  A plot of the contact force history is sought. 
this  problem
Figure 16.1 – Finite element model with selected parts, 
elements, and nodes identified. 
Analysis Summary: 
Dim. 
Type 
Load  Material  Geometry  Contact 
Solver 
2D  Dynamic  Gravity  Linear 
Linear 
2D 
Implicit 
Solution 
Method 
2-Nonlinear 
w/BFGS 
Units: 
lbf-s2/in, in, s, lbf, psi, lbf-in (blob, inch, second, pound force, pound force/inch2, 
pound force-inch) 
Dimensional Data: 
=
×
1.0 10
in
, 
=
×
1.0 10
Material Data: 
Mass Density 
Nodal Mass 
ρ=
=
3.995281 10
×
0.50
lbf
−
/
in
lbf
−
/
in
Spring Stiffness 
=
1.97392 10
×
lb in
/
Load: 
Body Force 
Element Types: 
=
=
=
=
0.0
in s
/
0.0
in s
/
×
3.86 10
×
3.86 10
 varied linearly to 3.86 10
×
in s
/
, then held constant
,
=
0.0
/
in s
in s
/
,
,
=
=
×
1.0 10
×
1.0 10
s−
2D plane strain shell element (xy plane) - *SECTION_BEAM entry (elform=7) 
Plane strain (x-y plane) - *SECTION_SHELL entry - (elform=13) 
Translational spring - (SECTION_DISCRETE (dro=0) 
Material Models: 
*MAT_001 or *MAT_ELASTIC 
*MAT_020 or *MAT_RIGID 
Results Comparison: 
LS-DYNA results for velocity  YV  and displacement 
(plus the time) and maximum displacement of the cylindrical disk 
with W.T. Thomson's studies in Vibration Theory and Applications, 1965 (pg. 110). 
YU  of the cylindrical disk at impact 
, are compared 
YmaxU
Impact 
Time (s) 
Velocity 
YV  (in/s) 
Displacement 
YU  (in) 
Max. Disp. 
 (in) 
YmaxU
0.07198 
-27.7900 
-1.0000 
-1.5506 
0.07240 
-27.7728 
-0.9978 
-1.5524 
Thomson 
[1965] 
Cylindrical
LS-DYNA  results  are  reported  at  the  closet  time  point  for  the  displacement  value 
= −
designated as full stiffness contact (i.e. 
1.0000
 in). 
YU
The  nodal  results  were  generated  by  *DATABASE_NODOUT  keyword,  the  kinetic 
energy by *DATABASE_MATSUM keyword, and the contact force by *DATABASE_ 
RCFORC keyword. 
Figure 16.2 provides  the velocity 
history, and Figure 16.4 the kinetic energy history, all of the cylindrical disk. 
YV  history,  Figure 16.3  the vertical displacement 
YU  
Figure 16.5 gives the contact force between the cylindrical disk (slave) and the flexible 
surface (master).
Figure 16.3 – Vertical displacement 
YU  of the cylindrical disk.
Figure 16.5 – Contact force between cylindrical disk (slave) 
and flexible surface (master). 
Input deck: 
*KEYWORD 
*TITLE 
Transient Response of a Cylindrical Disk Impacting a Flexible Surface 
*CONTROL_IMPLICIT_DYNAMICS 
$#   imass     gamma      beta 
         1  0.500000  0.250000 
*CONTROL_IMPLICIT_AUTO 
$#   iauto    iteopt    itewin     dtmin     dtmax 
         1        11         5  1.00e-06  1.00e-04 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form 
         1  0.000100         0         0         0 
*CONTROL_IMPLICIT_SOLVER 
$#  lsolvr   prntflg    negeig     order      drcm    drcprm   autospc    aspctl 
         4         2         2         0         1         0         1         0 
$#  lcpack 
         2 
*CONTROL_IMPLICIT_SOLUTION 
$#  nsolvr    ilimit    maxref     dctol     ectol     rctol     lstol    abstol 
         2        11        15    0.0010    0.0100  1.00e+10  0.900000  1.00e-10 
$#   dnorm    diverg     istif   nlprint    nlnorm   d3itctl     cpchk 
         2         1         1         2 
$#  arcctl    arcdir    arclen    arcmth    arcdmp 
         0         1       0.0         1         2 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
    0.1100 
*DATABASE_GLSTAT
$#      dt    binary 
1.0000e-04         1 
*DATABASE_RCFORC 
$#      dt    binary 
1.0000e-04         1 
*DATABASE_NODOUT 
$#      dt    binary 
1.0000e-04         1 
*DATABASE_BINARY_D3PLOT 
$# dt/cycl   lcdt/nr      beam     npltc    psetid 
1.0000e-03 
*DATABASE_HISTORY_NODE 
$#    nid1      nid2      nid3      nid4       ni5      nid6      nid7      nid8 
       166      1001 
*PART 
$# title                                                                         
rigid cylindrical disk 
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1 
*SECTION_SHELL 
$#   secid    elform      shrf       nip     propt   qr/irid     icomp     setyp 
         1        13         0         4 
$#      t1        t2        t3        t4      nloc     marea      
    1.0000    1.0000    1.0000    1.0000 
*MAT_RIGID 
$      mid        ro         e        pr         n    couple         m     alias 
         1 3.9952831  3.00e+07    0.3000       0.0       0.0       0.0       0.0 
$      cmo      con1      con2 
    1.0000       6.0       7.0 
$lco_or_a1        a2        a3        v1        v2        v3 
       0.0       0.0       0.0       0.0       0.0       0.0 
*PART 
discrete spring - flexible surface 
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         2         2         2 
*SECTION_DISCRETE 
$#   secid       dro        kd        v0        cl        fd 
         2         0         0         0       0.0       0.0 
$#     cdl       tdl 
       0.0       0.0 
*MAT_SPRING_ELASTIC 
$#     mid         k 
         2 1973.9200 
*PART 
rigid plane beam (wall) 
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         3         3         3 
*SECTION_BEAM 
$#   secid    elform      shrf   qr/irid       cst     scoor      nsm 
         3         7    1.0000    1.0000    0.0000 
$      ts1       ts2       tt1       tt2 
    0.1000    0.1000 
*MAT_RIGID 
$      mid        ro         e        pr         n    couple         m     alias 
         3  1.00e-07  3.00e+07    0.3000       0.0       0.0       0.0       0.0 
$      cmo      con1      con2 
    1.0000       6.0       7.0 
$lco_or_a1        a2        a3        v1        v2        v3 
       0.0       0.0       0.0       0.0       0.0       0.0 
*ELEMENT_BEAM 
    1002       3    1003    1001 
    1003       3    1001    1004 
*ELEMENT_DISCRETE 
$    eid     pid      n1      n2     vid               s      pf          offset 
    1001       2    1001    1002       0             1.0       0             0.0 
*ELEMENT_SHELL 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8
$#   nid               x               y               z      tc      rc 
       1     -0.14142136      0.05857864             0.0 
     521      0.16180338      0.31755710             0.0 
    1001             0.0          -1.050             0.0       6       7 
    1002             0.0          -2.050             0.0       7       7 
    1003            -0.5          -1.050             0.0       6       7 
    1004             0.5          -1.050             0.0       6       7 
$    1001             0.0            -1.0             0.0       6       7 
$    1002             0.0            -2.0             0.0       7       7 
$    1003            -0.5            -1.0             0.0       6       7 
$    1004             0.5            -1.0             0.0       6       7 
*CONTACT_2D_AUTOMATIC_NODE_TO_SURFACE 
$#    ssid      msid     sfact      freq        fs        fd        dc     membs 
        -2        -1      0.10         0         0         0         0         0 
$#  tbirth    tdeath       sos       som       nds       ndm       cof      init 
         0         0         0         0         0         0         0         0 
$#      vc       vdc       ipf     slide    istiff   tiedgap 
                                                 2 
$*CONTACT_2D_PENALTY 
$#    ssid      msid    tbirth    tdeath 
$         2         1 
$# ext_pas    theta1    theta2    tol_ig       pen    toloff    frcscl    oneway 
$                                              0.10   0.00010 
*SET_NODE_LIST 
$#     sid       da1       da2       da3       da4 
         1 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
      1003      1001      1004 
*SET_NODE_LIST 
$#     sid       da1       da2       da3       da4 
         2 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
       155       166       177 
*LOAD_BODY_Y 
$     lcid        sf    lciddr        xc        yc        zc       cid 
         1       1.0 
*DEFINE_CURVE 
$#    lcid      sdir       sfa       sfo      offa      offo    dattyp 
         1         0    1.0000    1.0000       0.0       0.0 
$#                a1                  o1 
               0.000               0.000 
               0.001              386.00 
               1.000              386.00 
*END 
Notes: 
1.  From the LS-DYNA User's Manual: Note that the 2D and 3D element types must not 
be  mixed,  and  different  types  of  2D  elements,  i.e.  plane  strain,  plane  stress,  and 
axisymmetric,  must  not  be  used  together.    The  discrete  (spring)  1D  element  can  be 
used with either 2D or 3D elements. 
2.  Consider the two surfaces comprising a contact.  It is necessary to designate one as a 
slave  surface  and  the  other  as  a  master  surface.    Nodal  points  defining  the  slave 
surface  are  called  slave  nodes,  and  similarly,  nodes  defining  the  master  surface  are 
called  master  nodes.    Each  slave-master  surface  combination  is  referred  to  as  a 
contact surface.  If one surface is more finely zoned, it should be defined as the slave
3.  By  default,  the  true  thickness  of  2D  shell  elements  is  taken  into  account  for 
*CONTACT_2D _AUTOMATIC_SURFACE_TO_SURFACE and _AUTOMATIC_ 
NODE_TO_SURFACE contacts.  The user can override the true thickness by using 
the sos and som parameters on the contact entry. 
input example: 
*CONTACT_2D_AUTOMATIC_NODE_TO_SURFACE 
$#    ssid      msid     sfact      freq        fs        fd        dc     membs 
        -2        -1      0.10         0         0         0         0         0 
$#  tbirth    tdeath       sos       som       nds       ndm       cof      init 
         0         0         0         0         0         0         0         0 
$#      vc       vdc       ipf     slide    istiff   tiedgap 
                                                 2 
$ 
*SET_NODE_LIST 
$#     sid       da1       da2       da3       da4 
         1 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
      1003      1001      1004 
*SET_NODE_LIST 
$#     sid       da1       da2       da3       da4 
         2 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
       155       166       177 
$ 
*NODE 
$#   nid               x               y               z      tc      rc 
    1001             0.0          -1.050             0.0       6       7 
    1002             0.0          -2.050             0.0       7       7 
    1003            -0.5          -1.050             0.0       6       7 
    1004             0.5          -1.050             0.0       6       7 
There is a stiffness control variable available, cof, which allows the full stiffness to be 
gradually  applied  as  a  node  approaches  a  segment.    The  tolerance  for  the  stiffness 
appears  to  be  hardwired  internally  in  the  LS-DYNA  software.    cof  offers  only  two 
options: on (cof=0 - LS-DYNA default) or off (cof=1); no tolerance adjusting. 
  Using cof=0 activates the  contact stiffness as a node  approaches a segment  at some 
unknown  value;  the  stiffness  is  increased  as  the  node  moves  closer  with  the  full 
stiffness being used when the  nodal  point finally makes  contact.   Using  cof=1 does 
not turn on any contact stiffness until the nodal point makes full stiffness contact. 
It is observed that the contact output force  calculation (*DATABASE_RCFORC) is 
not made (delayed) until full stiffness contact is made for either cof option. 
For cof=1, the contact force is calculated without a delay (due to full stiffness being 
applied  without  the  gradual  increase),  but  is  nosier  (oscillatory)  than  the  other 
solution cof=0, at least for this example problem. 
4.  If  the  older  penalty  contact  algorithms  are  used,  *CONTACT_2D  _PENALTY  and 
_PENALTY_ FRICTION, the  slave-master distinction is irrelevant.  These contacts 
use the mid-surface of the 2D shell elements; thus, the shell thickness is not taken into
coordinates  to  achieve  reasonable  results,  e.g.,  the  arrival  time  of  a  dropped  rigid 
sphere onto a 2D shell plate of a moderate thickness. 
input example: 
*CONTACT_2D_PENALTY 
$#    ssid      msid    tbirth    tdeath 
         2         1 
$# ext_pas    theta1    theta2    tol_ig       pen    toloff    frcscl    oneway 
                                              0.10   0.00010 
       155       166       177 
$ 
*SET_NODE_LIST 
$#     sid       da1       da2       da3       da4 
         1 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
      1003      1001      1004 
*SET_NODE_LIST 
$#     sid       da1       da2       da3       da4 
         2 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
       155       166       177 
$ 
*NODE 
$#   nid               x               y               z      tc      rc 
    1001             0.0            -1.0             0.0       6       7 
    1002             0.0            -2.0             0.0       7       7 
    1003            -0.5            -1.0             0.0       6       7 
    1004             0.5            -1.0             0.0       6       7 
There  is  an  adjustable,  stiffness  control  variable  available,  toloff,  which  allows  the 
full stiffness to be gradually applied as a node approaches a segment. 
From  the  LS-DYNA  User's  Manual:  toloff  -  Tolerance  for  stiffness  activation  for 
implicit solution only.    The  contact stiffness is  activated when  a node approaches a 
segment at a distance equal to the segment length multiplied by toloff.  The stiffness 
is increased as the node moves closer with the full stiffness being applied when the 
nodal point finally makes contact. 
It is observed that the contact output force calculation (*DATABASE_RCFORC) is
17.  Natural Frequency of a Linear Spring-Mass System 
Keywords: 
*CONTROL_TIMESTEP 
*ELEMENT_DISCRETE 
*ELEMENT_MASS 
*MAT_SPRING_ELASTIC 
Description: 
A mass (m) is attached to a linear spring, as shown in Figure 17.1.  The mass is initially 
= −
displaced 
 from its equilibrium position and released.  Determine the period 
of vibration τ. 
1.0
in
The spring is modeled by one discrete element (*ELEMENT_DISCRETE) using a linear 
elastic  spring  material  (*MAT_S01/*MAT_SPRING_ELASTIC).    The  lumped  mass  is 
modeled by an *ELEMENT_MASS entry. 
Figure 17.1 – Sketch representing the model. 
Analysis Summary: 
Dim. 
Type 
Load  Material  Geometry  Contact 
Solver 
Solution 
Method 
3D  Dynamic 
Initially 
Displace 
Linear 
Linear 
- 
Explicit
Units: 
lbf-s2/in, in, s, lbf, psi, lbf-in (blob, inch, second, pound force, pound force/inch2, 
pound force-inch) 
Dimensional Data: 
=
×
1.0 10
in
Material Data: 
Nodal Mass 
Spring Stiffness 
Element Types: 
−
=
=
×
2.588 10
in
lbf
5.0
/
lbf
−
/
in
Translational spring - *SECTION_DISCRETE (dro=0) 
Lumped mass (*ELEMENT_MASS entry) 
Material Models: 
*MAT_S01 or *MAT_SPRING_ELASTIC 
Results Comparison: 
LS-DYNA results for the period of vibration related to this linear spring-mass system are 
compared  with  S.P.  Timoshenko  and  D.H.  Young  studies  in  Vibration  Problems  in 
Engineering, 1955 (pg. 1). 
Timoshenko and Young [1955] 
Linear spring-mass system 
Period of Vibration τ (s) 
0.14295 
0.14295 
This  nodal  displacement  result  and  the  computer  period  of  vibration  was  generated  by
Figure 17.2 – Node 1 displacement UY .
*TITLE 
Natural Frequency of a Linear Spring-Mass System 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
  0.150000         0       0.0       0.0       0.0 
*CONTROL_TIMESTEP 
$#  dtinit    tssfac      isdo    tslimt     dt2ms      lctm     erode     ms1st 
 1.000e-04 1.000e-04         0       0.0       0.0         0         0         0 
$#  dt2msf   dt2mslc     imscl 
       0.0         0         0 
*DATABASE_NODOUT 
$#      dt    binary 
  0.000100 
*DATABASE_BINARY_D3PLOT 
$# dt/cycl   lcdt/nr      beam     npltc    psetid 
  0.001000 
*DATABASE_HISTORY_NODE 
$#    nid1      nid2      nid3      nid4       ni5      nid6      nid7      nid8 
         1 
*PART 
$# title                                                                         
linear elastic spring                                                         
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1 
*SECTION_DISCRETE 
$#   secid       dro        kd        v0        cl        fd 
         1         0       0.0       0.0       0.0       0.0 
$#     cdl       tdl 
       0.0       0.0 
*MAT_SPRING_ELASTIC 
$#     mid         k 
         1      5.00 
*ELEMENT_DISCRETE 
$#   eid     pid      n1      n2     vid               s      pf          offset 
       1       1       1       2       0         1.00000       0         1.00000 
*ELEMENT_MASS 
$#   eid      id            mass     pid 
       2       1      0.00258800 
       3       2      0.00258800 
*NODE 
$#   nid               x               y               z      tc      rc 
       1             0.0             0.0             0.0 
       2             0.0      1.00000000             0.0 
*BOUNDARY_SPC_NODE 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         2         0         1         1         1         1         1         1 
*END 
Notes: 
1.  As an alternative, it is possible to model the linear spring with a *BEAM_ELEMENT 
the  option  discrete)  and  *MAT_066/*MAT_  LINEAR_ELASTIC_ 
(with
2.  For simulations with linear stiffness, one could use the following implicit entries and 
perform a simple eigenvalue analysis: 
*CONTROL_IMPLICIT_EIGENVALUE 
$#    neig    center     lflag    lftend     rflag    rhtend    eigmth    shfscl 
         3    11.000         0 -1.00e+29         0  1.00e+29         2       0.0 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form 
         6  1.00e-04         2         1         2 
The  period  could  be  obtained  directly  from  the  eigout  results  file  generated  by  the 
*CONTROL_IMPLICIT_EIGENVALUE keyword as shown here: 
Natural Frequency of a Linear Spring-Mass System                      
r e s u l t s   o f   e i g e n v a l u e   a n a l y s i s: 
                             |------ frequency -----| 
        MODE    EIGENVALUE       RADIANS        CYCLES        PERIOD 
           1   4.547474E-12   2.132481E-06   3.393948E-07   2.946421E+06 
           2   5.456968E-12   2.336015E-06   3.717884E-07   2.689702E+06
18.  Natural Frequency of a Nonlinear Spring-Mass System 
Keywords: 
*CONTROL_TIMESTEP 
*ELEMENT_DISCRETE 
*ELEMENT_MASS 
*MAT_SPRING_NONLINEAR_ELASTIC 
Description: 
A  mass  (m)  is  attached  to  a  nonlinear  spring: 
= −
The  mass  is  initially  displaced 
Determine the period of vibration τ. 
1.0
in
=
+
δk
,  as  shown  in  Figure  18.1.  
  from  its  equilibrium  position  and  released.  
The  spring  is  modeled  by  one  discrete  element  (*ELEMENT_DISCRETE)  using  a 
nonlinear 
(*MAT_S04/*MAT_SPRING_NONLINEAR_ 
ELASTIC).  The lumped mass is modeled by an *ELEMENT_MASS entry. 
spring  material 
elastic 
To  input  the  data  for  the  *MAT_S04/*MAT_SPRING_NONLINEAR_ELASTIC  it  is 
( )δF
: 
necessary  to  convert  the  stiffness-deflection  curve 
, using a *DEFINE_CURVE entry.  This curve is converted to eleven 
. 
=
F k
points of force-deflection points in the range 
  to  a  force-deflection 
δ δ δ
]1,0[=δ
( )δk
+
=
Analysis Summary: 
Dim. 
Type 
Load  Material  Geometry  Contact 
Solver 
Solution 
Method 
3D  Dynamic 
Initially 
Displace 
Non-
linear 
Linear 
- 
Explicit 
- 
Units: 
lbf-s2/in, in, s, lbf, psi, lbf-in (blob, inch, second, pound force, pound force/inch2, 
pound force-inch) 
Dimensional Data: 
=
×
1.0 10
in
Material Data: 
Nodal Mass 
Spring Stiffness 
=
=
Element Types: 
−
×
2.588 10
δk
, 
+
lbf
=
−
2.0
/
in
lbf
/
in
, 
=
4.0
lbf
/
in
Translational spring - *SECTION_DISCRETE (dro=0) 
Lumped mass (*ELEMENT_MASS entry) 
Material Models: 
*MAT_S04 or *MAT_SPRING_NONLINEAR_ELASTIC 
Results Comparison: 
LS-DYNA results for the period of vibration related to this nonlinear spring-mass system 
are  compared  with  S.P.  Timoshenko  and  D.H.  Young  studies  in  Vibration  Problems  in 
Engineering, 1955 (pg. 141). 
Timoshenko and Young [1955] 
Nonlinear spring-mass system 
Period of Vibration τ (s) 
0.14470
This  nodal  displacement  result  and  the  computer  period  of  vibration  was  generated  by 
*DATABASE_NODOUT keyword (also see Figures 18.2 and 18.3). 
Figure 18.2 – Node 1 displacement UY .
*TITLE 
Natural Frequency of a Nonlinear Spring-Mass System 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
  0.150000         0       0.0       0.0       0.0 
*CONTROL_TIMESTEP 
$#  dtinit    tssfac      isdo    tslimt     dt2ms      lctm     erode     ms1st 
 1.000e-04 1.000e-04         0       0.0       0.0         0         0         0 
$#  dt2msf   dt2mslc     imscl 
       0.0         0         0 
*DATABASE_NODOUT 
$#      dt    binary 
  0.000100 
*DATABASE_BINARY_D3PLOT 
$# dt/cycl   lcdt/nr      beam     npltc    psetid 
  0.001000 
*DATABASE_HISTORY_NODE 
$#    nid1      nid2      nid3      nid4       ni5      nid6      nid7      nid8 
         1 
*PART 
$# title                                                                         
nonlinear elastic spring                                                         
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1 
*SECTION_DISCRETE 
$#   secid       dro        kd        v0        cl        fd 
         1         0       0.0       0.0       0.0       0.0 
$#     cdl       tdl 
       0.0       0.0 
*MAT_SPRING_NONLINEAR_ELASTIC 
$#     mid       lcd       lcr 
         1         1 
*DEFINE_CURVE 
$#    lcid      sdir       sfa       sfo      offa      offo     dattyp 
         1         0  1.000000  1.000000       0.0       0.0 
$#                a1                  o1 
                0.00              0.0000 
                0.10              0.2040 
                0.20              0.4320 
                0.30              0.7080 
                0.40              1.0240 
                0.50              1.5000 
                0.60              2.0640 
                0.70              2.7720 
                0.80              3.6480 
                0.90              4.7160 
                1.00              6.0000 
*ELEMENT_DISCRETE 
$#   eid     pid      n1      n2     vid               s      pf          offset 
       1       1       1       2       0         1.00000       0         1.00000 
*ELEMENT_MASS 
$#   eid      id            mass     pid 
       2       1      0.00258800 
       3       2      0.00258800 
*NODE 
$#   nid               x               y               z      tc      rc 
       1             0.0             0.0             0.0 
       2             0.0      1.00000000             0.0 
*BOUNDARY_SPC_NODE 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         2         0         1         1         1         1         1         1
Notes: 
1.  A somewhat better comparison could be achieved with a more detailed representation 
of the nonlinear spring stiffness. 
2.  As  an  alternative, 
*BEAM_ELEMENT 
NONLINEAR_ELASTIC_DISCRETE_BEAM material behavior. 
the  option  discrete) 
is  possible 
to  model 
the  nonlinear  spring  with  a 
and  *MAT_067/*MAT_ 
(with 
it 
3.  For simulations with linear stiffness, one would use the following implicit entries and 
perform a simple eigenvalue analysis: 
*CONTROL_IMPLICIT_EIGENVALUE 
$#    neig    center     lflag    lftend     rflag    rhtend    eigmth    shfscl 
         3    11.000         0 -1.00e+29         0  1.00e+29         2       0.0 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form 
         6  1.00e-04         2         1         2 
The  period  could  be  obtained  directly  from  the  eigout  results  file  generated  by  the 
*CONTROL_IMPLICIT_EIGENVALUE keyword as shown here: 
Natural Frequency of a Nonlinear Spring-Mass System                      
r e s u l t s   o f   e i g e n v a l u e   a n a l y s i s: 
                             |------ frequency -----| 
        MODE    EIGENVALUE       RADIANS        CYCLES        PERIOD 
           1  -9.094947E-11   9.536743E-06   1.517820E-06   6.588397E+05 
           2   4.547474E-12   2.132481E-06   3.393948E-07   2.946421E+06 
           3   4.961360E+03   7.043692E+01   1.121038E+01   8.920301E-02 
However,  for  this  example,  the  spring  stiffness  is  nonlinear,  represented  by  a 
piecewise  linear  curve.    LS-DYNA  will  make  a  stiffness,  from  two  force-
displacement  pairs,  to  compute  an  eigenvalue.    Which  pairs  used  will  depend  on 
whether  there is  an initial offset or  not (provided via *ELEMENT_DISCRETE).   If 
there is zero initial offset, the first two force-displacement pairs are used; if there is an 
initial offset, the two pairs on either side of the offset would be used; if the offset and 
displacement  value  are  equal,  LS-DYNA  uses  this  as  the  upper  pair.    Using  this 
stiffness value will not yield a correct period of vibration.
19.  Buckling of a Axially Loaded Thin Walled Cylinder 
Keywords: 
*CONTROL_IMPLICIT_GENERAL 
*CONTROL_IMPLICIT_SOLUTION 
*CONTROL_IMPLICIT_BUCKLE 
*CONTROL_IMPLICIT_EIGENVALUE 
Description: 
A  cylinder  is  loaded  with  a  uniform  distributed  (equal  value  to  each  node)  line  load  of 
P 1000
 (compressive) along the top edge. Determine the critical buckling load. 
lbs
=
The  lower  end  of  the  cylinder  is  clamped,  i.e.  fixed  for  all  translational  and  rotational 
= , the upper end of the cylinder is only 
=
0=z
directions (
= ). 
fixed in x and y direction (
=
=
z = : 
=
U=
: 
=
The finite element model is shown in Figure 19.1. 
Figure 19.1 – Finite element model with applied axial load and boundary nodes
Analysis Type: 
Dim. 
Type 
Load  Material  Geometry  Contact 
Solver 
3D 
Static 
Force 
Linear 
Linear 
- 
Implicit 
Solution 
Method 
2-Nonlinear 
w/BFGS 
Units: 
lbf-s2/in, in, s, lbf, psi, lbf-in (blob, inch, second, pound force, pound force/inch2, 
pound force-inch) 
Dimensional Data: 
=
×
1.20 10
in
, 
cr
=
×
4.8 10
in
, 
=
×
1.0 10
in−
Material Data: 
Mass Density 
Young's Modulus 
Poisson's Ratio 
=
=
ν =
Load: 
−
lbf
−
/
in
lbf
/
in
×
1.00 10
×
1.00 10
0.3
Axial Load 
=
×
1.00 10
lbs
Element Types: 
Belytschko-Tsay shell (elform=2) 
S/R Hughes-Liu shell (elform=6) 
Belytschko-Wong-Chiang shell (elform=10) 
Fully integrated shell (elform=16) 
Material Models: 
*MAT_001 or *MAT_ELASTIC 
Results Comparison: 
LS-DYNA  results  for  the  critical  buckling  load  of  a  thin  walled  cylinder  under  axial 
compression  are  compared  with  S.P.  Timoshenko  and  J.M.  Gere  studies  in  Theory  of
Critical Buckling 
Load 
crP (lbf) 
Critical Axial 
σ (psi) 
Stress  cr
Timoshenko and Gere [1961] 
3.8025 10×
1.2608 10×
Belytschko-Tsay shell (elform=2) 
3.8763 10×
1.2853 10×
S/R Hughes-Liu shell (elform=6) 
4.6226 10×
1.5327 10×
Belytschko-Wong-Chiang shell (elform=10) 
3.8763 10×
1.2853 10×
Fully integrated shell (elform=16) 
4.6086 10×
1.5281 10×
The analytical solution for this problem, from Timoshenko and Gere [1961], is: 
*
cr
=
(
3 1
−
)
=
1.2608 10
×
psi
with a mode shape that is sinusoidal both axially and circumferentially. 
The  LS-DYNA  critical  load 
axial load: 
crP   is  computed  from  the  first  eigenvalue  and  the  applied 
crP
λ=
=
3.8762 10
×
×
1.0000 10
×
lbf
=
3.8762 10
×
lbf
while the critical axial stress 
crσ  is given by 
cr
=
cr
=
3.8763 10
3.0159 10
×
×
lbf
in
=
1.2853 10
×
psi
This result, for the one point quadrature shell elements (elform=2 and elform=10), is in 
good agreement with the analytical solution. 
The  critical  load  and  axial  stress  for  the  fully  integrated  shell  elements  (elform=6  and 
elform=16) is greater than the one point quadrature shell elements.  The difference is not
Eigenvalue Results: 
From the eigout file, generated by the *CONTROL_IMPLICIT_BUCKLE keyword: 
Belytschko-Tsay shell (elform=2): 
Buckling of a Thin Walled Cylinder Under Compression                     
r e s u l t s   o f   e i g e n v a l u e   a n a l y s i s: 
                             |------ frequency -----| 
        MODE    EIGENVALUE       RADIANS        CYCLES        PERIOD 
           1   3.876317E+02 
           2   3.882852E+02 
           3   3.882852E+02 
S/R Hughes-Liu shell (elform=6) 
Buckling of a Thin Walled Cylinder Under Compression                     
r e s u l t s   o f   e i g e n v a l u e   a n a l y s i s: 
                             |------ frequency -----| 
        MODE    EIGENVALUE       RADIANS        CYCLES        PERIOD 
           1   4.622332E+02 
           2   4.622523E+02 
           3   4.700114E+02 
Belytschko-Wong-Chiang shell (elform=10) 
Buckling of a Thin Walled Cylinder Under Compression                     
r e s u l t s   o f   e i g e n v a l u e   a n a l y s i s: 
                             |------ frequency -----| 
        MODE    EIGENVALUE       RADIANS        CYCLES        PERIOD 
           1   3.876317E+02 
           2   3.882852E+02 
           3   3.882852E+02 
Fully integrated shell (elform=16) 
Buckling of a Thin Walled Cylinder Under Compression                     
r e s u l t s   o f   e i g e n v a l u e   a n a l y s i s: 
                             |------ frequency -----| 
        MODE    EIGENVALUE       RADIANS        CYCLES        PERIOD 
           1   4.608551E+02 
           2   4.608564E+02 
           3   4.681777E+02 
The  one  point  quadrature  shell  elements  (elform  =2  and  elform=10)  only  provide  the 
axial sinusoidal mode shape (10 half sine waves) as can be seen in Figure 19.2. 
The fully integrated shell elements (elform=6 and elform=16) provide both the axial and 
circumferential sinusoidal mode shapes (2 half sine waves axially and 20 half sine waves 
circumferentially) as can be seen in Figure 19.3. 
The  eigenmodes  for  the  one  point  quadrature  elements  and  the  fully  integrated  shell
Figure 19.2 – First eigenmode with the 1000 lbf load applied (elform=10).
*TITLE 
Buckling of a Thin Walled Cylinder Under Compression 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form 
         1  0.100000         2         1         2 
*CONTROL_IMPLICIT_SOLUTION 
$#  nsolvr    ilimit    maxref     dctol     ectol  not used     lstol      rssf 
         2        11        15  0.001000  0.010000       0.0  0.900000  1.000000 
$#   dnorm    diverg     istif   nlprint 
         2         1         1         2 
$#  arcctl    arcdir    arclen    arcmth    arcdmp 
         0         1       0.0         1         2 
*CONTROL_IMPLICIT_BUCKLE 
$#   nmode 
         3 
*CONTROL_IMPLICIT_EIGENVALUE 
$#    neig    center     lflag    lftend     rflag    rhtend    eigmth    shfscl 
                                                                           300.0 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
  1.000000         0       0.0       0.0       0.0 
*CONTROL_SHELL 
$#  wrpang     esort     irnxx    istupd    theory       bwc     miter      proj 
  20.00000         0         0         0         2         1         1         1 
$# rotascl    intgrd    lamsht    cstyp6    tshell    nfail1    nfail4 
       0.0         0 
*DATABASE_BINARY_D3PLOT 
$# dt/cycl 
  0.010000 
*PART 
$# title                                                                         
material type # 1  (Elastic)                                                     
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1         0         1 
*SECTION_SHELL 
$#   secid    elform      shrf       nip     propt   qr/irid     icomp     setyp 
         1         2       0.0         0         1       0.0         0         1 
$         1         6       0.0         0         1       0.0         0         1 
$         1        10       0.0         0         1       0.0         0         1 
$         1        16       0.0         0         1       0.0         0         1 
$#      t1        t2        t3        t4      nloc     marea 
  0.100000  0.100000  0.100000  0.100000         0       0.0 
*MAT_ELASTIC 
$#     mid        ro         e        pr        da        db  not used 
         1  0.0100001.0000e+07  0.300000       0.0       0.0       0.0 
*HOURGLASS 
$#    hgid       ihq        qm       ibq        q1        q2        qb        qw 
         1         4       0.0         0       0.0       0.0       0.0       0.0 
*SET_NODE_LIST_TITLE 
bottom nodes 
$#     sid       da1       da2       da3       da4    solver 
         1       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nod4      nid5      nid6      nid7      nid8 
         1         2         3         4         5         6         7         8 
         9        10        11        12        13        14        15        16 
        17        18        19        20        21        22        23        24 
        25        26        27        28        29        30        31        32 
        33        34        35        36        37        38        39        40 
        41        42        43        44        45        46        47        48 
        49        50        51        52        53        54        55        56 
        57        58        59        60        61        62        63        64 
        65        66        67        68        69        70        71        72 
        73        74        75        76         0         0         0         0 
*SET_NODE_LIST_TITLE 
top nodes 
$#     sid       da1       da2       da3       da4    solver
$#    nid1      nid2      nid3      nod4      nid5      nid6      nid7      nid8 
      2205      2206      2207      2208      2209      2210      2211      2212 
      2213      2214      2215      2216      2217      2218      2219      2220 
      2221      2222      2223      2224      2225      2226      2227      2228 
      2229      2230      2231      2232      2233      2234      2235      2236 
      2237      2238      2239      2240      2241      2242      2243      2244 
      2245      2246      2247      2248      2249      2250      2251      2252 
      2253      2254      2255      2256      2257      2258      2259      2260 
      2261      2262      2263      2264      2265      2266      2267      2268 
      2269      2270      2271      2272      2273      2274      2275      2276 
      2277      2278      2279      2280         0         0         0         0 
*BOUNDARY_SPC_SET 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         1         0         1         1         1         1         1         1 
*BOUNDARY_SPC_SET 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         2         0         1         1         0         0         0         0 
*DEFINE_CURVE 
$#    lcid      sdir       sfa       sfo      offa      offo     dattyp 
         1         0       0.0       0.0       0.0       0.0 
$#                a1                  o1 
                 0.0                 0.0 
          1.00000000         13.15789474 
*LOAD_NODE_SET 
$#    nsid       dof      lcid        sf       cid        m1        m2        m3 
         2         3         1 -1.000000 
*ELEMENT_SHELL 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       1       2      78      77       0       0       0       0 
    2204       1    2204    2129    2205    2280       0       0       0       0 
*NODE 
$#   nid               x               y               z      tc      rc 
       1           0.000       48.000000           0.000       0       0 
    2280        3.963804       47.836056       120.00000       0       0 
*END 
Notes: 
1.  The keyword entry *CONTROL_IMPLICIT_BUCKLE allows for buckling analysis 
at the end of the static implicit simulation. 
2.  The  fully  integrated  and  one  point  quadrature  shell  elements  are  formulated  for 
nonlinear  analysis.    Although  this  analysis  is  linear,  it  was  solved  with  a  nonlinear
Mesh Convergence Study: 
Seven different mesh refinements were studied for this simulation: 
original mesh 29 axial by 76 circumferential elements (Figure 19.4a) 
•  
by 3.9671 10
4.1379 10
in
in
×
×
1st mesh refinement 58 axial by 152 circumferential elements 
×
•  
by 1.9840 10
2.0690 10
in
in
×
2nd mesh refinement 87 axial by 228 circumferential elements (Figure 19.4b) 
•  
by 1.3227 10
1.3793 10
in
in
×
×
3rd mesh refinement 116 axial by 304 circumferential elements 
•  
by 0.9921 10
1.0345 10
in
in
×
×
4th mesh refinement 145 axial by 380 circumferential elements (Figure 19.4c) 
•  
by 0.7937 10
0.8276 10
in
in
×
×
5th mesh refinement 174 axial by 456 circumferential elements 
×
•  
by 0.6614 10
0.6897 10
in
in
×
6th mesh refinement 203 axial by 532 circumferential elements 
•  
by 0.5669 10
0.5911 10
in
in
×
×
Figure 19.4a - Finite element model for the original mesh
Figure 19.4b - Finite element model for the 2nd mesh refinement 
(87 axial by 228 circumferential) discretization with applied axial load. 
Figure 19.4c - Finite element model for the 4th mesh refinement
Mesh Convergence Results Comparison: 
LS-DYNA  results  for  the  critical  buckling  load  of  a  thin  walled  cylinder  under  axial 
compression are compared for seven different mesh discretizations. 
analytical solution - 
3.8025 10×
 lbf 
Belytschko-Wong-
Chiang (elform=10) 
fully integrated 
shell (elform=16) 
original mesh 
(29 axial by 76 circumferential elements) 
3.8763 10×
4.6086 10×
1st mesh refinement 
(58 axial by 152 circumferential elements) 
3.8115 10×
4.0616 10×
2nd mesh refinement 
(87 axial by 228 circumferential elements) 
3.8052 10×
3.9313 10×
3rd mesh refinement 
(116 axial by 304 circumferential elements) 
3.8033 10×
3.8758 10×
4th mesh refinement 
(145 axial by 380 circumferential elements) 
3.8026 10×
3.8480 10×
5th mesh refinement 
(174 axial by 456 circumferential elements) 
3.8022 10×
3.8312 10×
6th mesh refinement 
(203 axial by 532 circumferential elements) 
3.8019 10×
3.8207 10×
For the Belytschko-Wong-Chiang (one point quadrature) shell element (elform=10), the 
29 axial by 76 circumferential element mesh (original) critical buckling load result was in 
good agreement with the analytical solution.  This element/mesh converged rapidly.  The 
29  axial  by  76  circumferential  element  mesh  only  differed  by  less  than  2%  from  the 
analytical solution while the 203 axial by 532 circumferential element mesh differed by 
less than 0.02%. 
For  the  fully  integrated  shell  element  (elform=16),  the  29  axial  by  76  circumferential 
element  mesh  (original)  critical  buckling  load  result  was  greater  (over  21%)  than  the 
analytical solution.  It is not known why.  Doubling the number of elements axially and 
circumferentially reduces the critical buckling by about 10%; however, still not in good 
agreement  with  the  analytical  solution,  especially  considering  the  level  of  mesh 
refinement.    Two  further  mesh  refinements  (116  axial  by  304  circumferential  element 
elements) were required to reach a similar good agreement (the 2% difference) with the 
one point quadrature shell element (elform=10) and the original mesh discretization.  The 
203 axial by  532  circumferential element mesh refinement for the fully integrated shell
The  one  point  quadrature  shell  element  (elform=10)  only  provides  the  axial  sinusoidal 
mode shape (Figures 19.5a and 19.5b): 
•   10 half sine waves in 29 axial by 76 circumferential element mesh (original), 
•   13 half sine waves in 58 axial by 152 circumferential element mesh, 
•   14 half sine waves in 87 axial by 228 circumferential element mesh, 
•   15 half sine waves in 116 axial by 304 circumferential element mesh, 
•   15 half sine waves in 145 axial by 380 circumferential element mesh, 
•   16 half sine waves in 174 axial by 456 circumferential element mesh, 
•   16 half sine waves in 203 axial by 532 circumferential element mesh, 
estimated from the eigenmode figures.  The number of half sine waves is the number of 
buckles.  It is not known why this element formulation only provides the axial sinusoidal
Figure 19.5a - First eigenmode with the 1000 lbf load applied for
Figure 19.5b - First eigenmode with the 1000 lbf load applied for the six
integrated  shell  element  (elform=16)  provides  both 
The  fully 
circumferential sinusoidal mode shapes (Figures 19.6a and 19.6b): 
•   2 half sine waves axially and 20 half sine waves circumferentially in 29 axial by 76 
the  axial  and 
circumferential element mesh (original), 
•   3 half sine waves axially and 24 half sine waves circumferentially in 58 axial by 152 
circumferential element mesh, 
•   4 half sine waves axially and 28 half sine waves circumferentially in 87 axial by 228 
circumferential element mesh, 
•   5 half sine waves axially and 30 half sine waves circumferentially in 116 axial by 304 
circumferential element mesh, 
•   6 half sine waves axially and 32 half sine waves circumferentially in 145 axial by 380 
circumferential element mesh, 
•   6 half sine waves axially and 32 half sine waves circumferentially in 174 axial by 456 
circumferential element mesh, 
•   7 half sine waves axially and 34 half sine waves circumferentially in 203 axial by 532 
circumferential element mesh.
Figure 19.6a - First eigenmode with the 1000 lbf load applied for
Figure 19.6b - First eigenmode with the 1000 lbf load applied for the six
Notes: 
1.  Solution problems may exist: 
•   because  LS-DYNA  buckling  solutions  assume  the  first  buckling  mode  will  be 
around 1.0 and/or 
•   if numerous eigenvalues are clustered around that smallest bucking frequencies. 
For  the  refined  meshes,  for  this  problem,  it  was  necessary  to  override  the  internal 
heuristic  for  picking  a  starting  point  for  Lanczos  shift  strategy,  which  is  the  initial 
Eigen  frequency  shift.    In  these  cases,  the  user  must  specify  the  initial  shift  via  the
20.  Membrane with a Hot Spot 
Keywords: 
*LOAD_THERMAL_LOAD_CURVE 
*MAT_ELASTIC_PLASTIC_THERMAL 
Description: 
This  benchmark  analyzes  the  behavior  of  shell  elements  subjected  to  a  thermal  load.  
Two  distinct  regions  are  modeled:  the  central  hot-spot  region  (radius  equal  to  r), 
subjected  to  the  thermal  strain 
,  and  the  rest  of  the  plate,  which  is  at  constant 
temperature  with 
.    Due  to  symmetry,  only  ¼  of  the  plate  (side  lengths  2L  and 
thickness t) is modeled (Figures 20.1a and 20.1b). 
Tαε =
ε=
0.0
The  material  defining 
is  *MAT_ELASTIC_PLASTIC_THERMAL 
(*MAT_004),  sensitive  to  temperature  changes.    The  rest  of  the  plate  is  defined  with 
material *MAT_ELASTIC (*MAT_001). 
the  hot  spot 
The  temperature  is  uniformly  applied  to  the  whole  model  by  means  of  the  *LOAD_ 
THERMAL_LOAD_CURVE keyword. 
Determine the y-component of the stress tensor along the edge y=0, just outside the hot 
spot. A fine mesh is required in the region of interest. 
To  possibly  achieve  better  accuracy,  the  value  at  the  integration  point  is  considered
Figure 20.1a - Finite element model (¼ symmetry) with 
selected nodes and dimensions identified. 
Figure 20.1b - Finite element model of hot spot (blue region) and refined
Analysis Summary: 
Dim.  Type 
Load  Material  Geometry  Contact 
Solver 
Solution 
Method 
3D 
Static 
Thermal  Linear 
Linear 
- 
Implicit 
1-Linear 
Units: 
ton ,mm, s, N, MPa, N-m,  C
millimeter, degree Centigrade) 
 (tonne, millmeter, second, Newton, MegaPascal, Newton-
Dimensional Data: 
=
10.0
mm
, 
=
1.00
mm
, 
=
1.00
mm
Material Data: 
Young's Modulus 
Poisson's Ratio 
Linear Expansion 
Load: 
Thermal 
Element Types: 
MPa
=
ν =
=
×
1.00 10
0.3
×
1.00 10
−
mm mm C
/
/

=
0.0 varied linearly to 100

Fully integrated shell (elform=16) 
Material Models: 
*MAT_001 or *MAT_ELASTIC 
*MAT_004 or *MAT_ELASTIC_PLASTIC_THERMAL 
Results Comparison: 
LS-DYNA global stress 
NAFEMS Background to Benchmark, Test T1.
Reference Condition - Point Just Outside 
Hot Spot (Node 18) 
Global Stress - σyy  (MPa) 
NAFEMS Benchmark Test T1 
Element 1148 (average value) 
First in-plane integration point (2x2 
quadrature) - element 1148 
Node 18 
5.0000 10×
4.7528 10×
4.5476 10×
4.3974 10×
YYσ   results  were  generated  from  *DATABASE_ELOUT  (elout  file) 
The  global  stress 
and *DATABASE_EXTENT_BINARY (eloutdet file provides detailed element output at 
integration points and connectivity nodes) keyword entries. 
You  can  set  intout=stress  or  intout=all  (*DATABASE_EXTENT_BINARY)  and  have 
file  called  eloutdet 
integration  points 
stresses  output 
(*DATABASE_ELOUT  governs  the  output  interval  and  *DATABASE_HISTORY_ 
SHELL governs which elements are output).  Setting nodout=stress or nodout=all all in 
*DATABASE_EXTENT_BINARY will write the extrapolated nodal stresses to eloutdet. 
for  all 
to  a 
the 
LS-DYNA stress and strain outputs correspond to integration point locations.  Stress at a 
node  is  an  artifact  of  the  post-processor  and  represents  an  average  of  the  surrounding 
integration point stresses (the value will likely be different with different postprocessors). 
Shell element stresses are reported at through-thickness integration points.  The location 
of those integration points depends on the  number  of  integration  points and the  type  of 
integration rule used, e. g., Gaussian, Lobatto, trapezoidal, user-defined rule .    Fully-integrated  shell  formulations  have  4  in-plane 
integration points at each through-thickness location. For these formulations, the 4 values 
of each stress component are averaged before being written to elout (except for the case 
of linear analysis when nsolvr=1 in *CONTROL_IMPLICIT_SOLUTION, in which case 
all 4 stress components are written to elout). 
Shell element stresses can be shown in the global, element, or material coordinate system.  
By default, shell element stresses/strains written to d3plot are global; shell stresses/strains 
written to elout are in the element local coordinate system (except for the case of linear 
analysis when nsolvr=1 in *CONTROL_IMPLICIT_SOLUTION, in which case stresses 
are in the global system).  Shell element stresses/strains from d3plot are converted by LS-
Even with this fine mesh in the region of interest, the large gradient temperature profile 
YYσ   along  the  line  of  symmetry.    The 
makes  it  difficult  to  capture  the  global  stress 
average  global  stress  of  the  element  (Figure  20.2)  provides  the  best  comparative  value 
(~5%  difference),  a  few  percent  better  than  the  nearest  element  integration  point  (~9% 
difference) and the extrapolated nodal (~12% difference) results. 
Figure 20.2 -Contour plot of global stress σyy .  Maximum value at element 1148. 
Input deck: 
*KEYWORD 
*TITLE 
Membrane with a Hot Spot 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form    zer0_v 
         1  0.100000         2         1         2         0         0         0 
*CONTROL_IMPLICIT_SOLUTION 
$#  nsolvr    ilimit    maxref     dctol     ectol     rctol     lstol    abstol 
         1        11        15  0.001000  0.010000   1.0e+10  0.900000  1.000000 
$#   dnorm    diverg     istif   nlprint    nlnorm    d3itcl     cpchk 
         2         1         1         0         2         0         0 
$#  arcctl    arcdir    arclen    arcmth    arcdmp    arcpsi    arcalf    arctim 
         0         0       0.0         1         2       0.0       0.0       0.0 
*CONTROL_SHELL 
$#  wrpang     esort     irnxx    istupd    theory       bwc     miter      proj 
  20.00000         0        -1         0        16         2         1         0 
$# rotascl    intgrd    lamsht    cstyp6    tshell 
  1.000000         0         0         1         0 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
  1.000000         0       0.0       0.0       0.0
$#   neiph     neips    maxint    strflg    sigflg    epsflg     rtflg    engflg 
         0         0         4         1         1         1         1         1 
$#  cmpflg    ieverp    beamip     dcomp      shge     stssz    n3thdt   ialemat 
$# nintsld   pkp_sen      sclp     hydro     msscl     therm    intout    nodout 
         1                 1.0                                  stress    stress 
*DATABASE_ELOUT 
$# dt/cycl 
  0.100000 
*DATABASE_HISTORY_SHELL 
$#    eid1      eid2      eid3      eid4       ei5      eid6      eid7      eid8 
      1148 
*DATABASE_GLSTAT 
$# dt/cycl 
  0.100000 
*DATABASE_MATSUM 
$# dt/cycl 
  0.100000 
*DATABASE_BINARY_D3PLOT 
$# dt/cycl 
  0.100000 
*PART 
$# title                                                                         
Part          1 for Mat         1 and Elem Type         16                       
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1 
*SECTION_SHELL 
$#   secid    elform      shrf       nip     propt   qr/irid     icomp     setyp 
         1        16  0.830000         1         1       0.0         0         1 
$#      t1        t2        t3        t4      nloc     marea 
  1.000000  1.000000  1.000000  1.000000         0       0.0 
*MAT_ELASTIC 
$#     mid        ro         e        pr        da        db  not used 
         1          1.0000e+05  0.300000       0.0       0.0       0.0 
*PART 
$# title                                                                         
Part          2 for Mat         2 and Elem Type         16                       
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         2         2         2 
*SECTION_SHELL 
$#   secid    elform      shrf       nip     propt   qr/irid     icomp     setyp 
         2        16  0.830000         1         1       0.0         0         1 
$#      t1        t2        t3        t4      nloc     marea 
  1.000000  1.000000  1.000000  1.000000         0       0.0 
*MAT_ELASTIC_PLASTIC_THERMAL 
$#     mid        ro 
         2 
$#      t1        t2        t3        t4        t5        t6        t7        t8 
       0.0  1000.000       0.0       0.0       0.0       0.0       0.0       0.0 
$#      e1        e2        e3        e4        e5        e6        e7        e8 
 1.000e+05 1.000e+05       0.0       0.0       0.0       0.0       0.0       0.0 
$#     pr1       pr2       pr3       pr4       pr5       pr6       pr7       pr8 
  0.300000  0.300000       0.0       0.0       0.0       0.0       0.0       0.0 
$#  alpha1    alpha2    alpha3    alpha4    alpha5    alpha6    alpha7    alpha8 
 1.000e-05 1.000e-05       0.0       0.0       0.0       0.0       0.0       0.0 
$#   sigy1     sigy2     sigy3     sigy4     sigy5     sigy6     sigy7     sigy8 
       0.0       0.0       0.0       0.0       0.0       0.0       0.0       0.0 
$#   etan1     etan2     etan3     etan4     etan5     etan6     etan7     etan8 
       0.0       0.0       0.0       0.0       0.0       0.0       0.0       0.0 
*ELEMENT_SHELL 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       2     344     368     441     345 
    1456       2     434     432     433     453 
*NODE 
$#   nid               x               y               z      tc      rc 
       1      1.00000000             0.0             0.0 
    1541      2.98852444      7.92062616             0.0 
*BOUNDARY_SPC_SET
3         0         0         1         1         1         1         1 
         4         0         1         0         1         1         1         1 
         5         0         1         1         1         1         1         1 
         6         0         0         0         1         1         1         0 
*SET_NODE_LIST_TITLE 
xsymm 
$#     sid       da1       da2       da3       da4    solver 
         3       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
        19        20       181       182       183       185       323       324 
       325       326       327       328       330       332        17       306 
       304       302       301       300       299       297       296       172 
       170       169       167        48        47        46        45        18 
         1        11        12       186       187       188       333       334 
       335       336       337       338         8       272       270       268 
       267       265       264       155       153       151        82        81 
*SET_NODE_LIST_TITLE 
ysymm 
$#     sid       da1       da2       da3       da4    solver 
         4       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
        36        83        84       147       150       154       257       258 
       261       262       269       271       316       315       312       311 
       308       307       177       175       173        38        37        33 
        89        90        91       130       135       137       140       221 
       224       231       232       235       236       239       242        65 
       282       279       278       277       276       275       274       273 
       160       158       157       156        68        67        66        61 
*SET_NODE_LIST_TITLE 
xy 
$#     sid       da1       da2       da3       da4    solver 
         5       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
        80 
*SET_NODE_LIST_TITLE 
whole 
$#     sid       da1       da2       da3       da4    solver 
         6       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         1         2         3         4         5         6         7         8 
      1537      1538      1539      1540      1541 
*LOAD_THERMAL_LOAD_CURVE 
$#    lcid    lciddr 
         1         0 
*DEFINE_CURVE 
$#    lcid      sdir       sfa       sfo      offa      offo     dattyp 
         1         0  1.000000  1.000000       0.0       0.0 
$#                a1                  o1 
                 0.0                 0.0 
          1.00000000         100.0000000 
*END 
Notes: 
1.  The fully integrated and one point quadrature shell elements are formulated for non-
linear analysis.  Although this analysis is linear, it could have been solved with a non-
linear solution method (nsolvr=2) which provides some slightly different stress output 
options .  This was done for this simulation and it was found to
21.  1D Heat Transfer with Radiation 
Keywords: 
*CONTROL_SOLUTION 
*CONTROL_THERMAL_SOLVER 
*CONTROL_THERMAL_NONLINEAR 
*CONTROL_THERMAL_TIMESTEP 
*BOUNDARY_TEMPERATURE_SET 
*BOUNDARY_RADIATION_SET 
*MAT_THERMAL_ISOTROPIC 
Description: 
A  0.10  m  long  bar  (
zL ),  with  square  0.01  m  (
yL )  cross-section  (Figure 
 at one end (node 
21.1), radiates  (steady state) to an ambient temperature of 
300
.  The bar 
11).  The other end (node 1) is maintained at constant temperature 
1000
is perfectly insulated along its length.  There is zero internal heat generation. 
xL )  x  0.01  m  (
=
=


Find the temperature at node 33 (x=0.000 m, y=0.010 m, z=0.100 m). 
The bar is meshed with 40 elements: ten elements along the length and four elements in 
the cross section.
Analysis Summary: 
Dim.  Type 
Load  Material  Geometry  Contact 
Solver 
3D 
Steady 
State 
Thermal  Linear 
Linear 
- 
Thermal 
Non-Linear 
Solution 
Method 
3-Diagonal 
scaled 
conjugate 
gradient 
Units: 
kg, m, s, N, Pa, N-m,  C

degree Centigrade) - Joule (J) is a N-m, Watt (W) is a J/s, 1
 (kilogram, meter, second, Newton, Pascal, Newton-meter, 

∆ = ∆
1C
Dimensional Data: 
xL
=
0.01
, 
yL
=
0.01
, 
zL
=
0.10
Material Data: 
Mass Density 
Heat Capacity 
Thermal Conductivity 
Emissivity 
ρ=
pC
=
ε=
×
7.850 10
=
4.600 10
×
×
5.560 10
0.980
/kg m

/
J kg C

W m C
/
Stefan-Boltzman 
=
5.670 10
×
−
/W m K

Load: 
Thermal 
Convection 
Initial Temperature 
Element Types: 

=
1000.0
×
=
7.500 10

=
300.0
 (constant) 
W m C
 (all nodes) 
/

Fully integrated S/R solid (elform=2) 
Material Models:
Results Comparison: 
LS-DYNA bar temperature at x=0.000 m, y=0.010 m, z= 0.100 m (Node 33) is compared 
with NAFEMS Background to Benchmark, Test T2. 
Reference Condition - Point Along Bar 
0.1 m (Node 33) from Hot End (Node 23) 
Temperature ( K
) 
NAFEMS Benchmark Test T2 
Node 33 
9.2700 10×
9.2700 10×
The fully integrated selectively reduced solid element (elform=2) model (also see Figure 
21.2) provides an exact temperature comparison for this coarse mesh. 
The problem is 1D, although solved in 3D.  The results are, as expected, the same for all 
x-y planes along the Z-direction.
*TITLE 
1D Heat Transfer with Radiation 
*CONTROL_SOLUTION 
$#    soln       nlq     isnan     lcint 
         1         0         0         0 
*CONTROL_THERMAL_SOLVER 
$#   atype     ptype    solver     cgtol       gpt    eqheat     fwork       sbc 
         0         1         3  1.00e-06         8  1.000000  1.0000005.6700e-08 
*CONTROL_THERMAL_NONLINEAR 
$#  refmax       tol       dcp 
        20 1.000e-06  0.500000 
*CONTROL_THERMAL_TIMESTEP 
$#      ts       tip       its      tmin      tmax     dtemp      tscp 
         1  0.500000 1.000e-04 1.000e-04  0.100000  1.000000  0.500000 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
   1.00000         0       0.0       0.0       0.0 
*DATABASE_TPRINT 
$#      dt    binary      lcur     ioopt 
  1.000000         0         0         1 
*DATABASE_HISTORY_NODE 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
        11        22        33        44        55        66        77        88 
        99 
*DATABASE_BINARY_D3PLOT 
$#      dt      lcdt      beam     npltc    psetid 
  1.000000         0         0         0         0 
*PART 
$# title                                                                         
Part          1 for TMat        1 and Elem Type         2                        
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         0         0         0         0         0         1 
*SECTION_SOLID 
$#   secid    elform       aet 
         1         2         1 
*MAT_THERMAL_ISOTROPIC 
$#    tmid       tro     tgrlc    tgmult 
         1  7850.000       0.0       0.0 
$#      hc        tc 
  460.0000   55.6000 
*BOUNDARY_TEMPERATURE_SET 
$#    nsid      lcid     cmult       loc 
         1         0  1000.000         0 
*BOUNDARY_RADIATION_SET 
$#    ssid      type 
         2         1 
$#   flcid     fmult    tilcid    timult       loc 
         05.5566e-08        0   300.0000         0 
*INITIAL_TEMPERATURE_SET 
$#    nsid      temp       loc 
         3  300.0000         0 
*SET_NODE_LIST_TITLE 
A 
$#     sid       da1       da2       da3       da4 
         1       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         1        12        23        34        45        56        67        78 
        89 
*SET_SEGMENT_TITLE 
B 
$#     sid       da1       da2       da3       da4 
         2     0.000     0.000     0.000     0.000 
$#      n1        n2        n3        n4        a1        a2        a3        a4 
        55        22        11        44     0.000     0.000     0.000     0.000 
        66        33        22        55     0.000     0.000     0.000     0.000 
        88        55        44        77     0.000     0.000     0.000     0.000
$#     sid       da1       da2       da3       da4 
         3       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         1         2         3         4         5         6         7         8 
         9        10        11        12        13        14        15        16 
        17        18        19        20        21        22        23        24 
        25        26        27        28        29        30        31        32 
        33        34        35        36        37        38        39        40 
        41        42        43        44        45        46        47        48 
        49        50        51        52        53        54        55        56 
        57        58        59        60        61        62        63        64 
        65        66        67        68        69        70        71        72 
        73        74        75        76        77        78        79        80 
        81        82        83        84        85        86        87        88 
        89        90        91        92        93        94        95        96 
        97        98        99 
*ELEMENT_SOLID 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       1      34      45      12       2      35      46      13 
      40       1      54      87      98      65      55      88      99      66 
*NODE 
$#   nid               x               y               z      tc      rc 
       1             0.0             0.0             0.0 
      99      0.01000000      0.01000000      0.10000000 
*END 
Notes: 
1.  The problem must be flagged as nonlinear if any boundary  condition parameter is a 
function  of  temperature.    This  includes  a  linear  (i.e.,  straight  line)  relationship.  
4T   boundary 
Iterations  are  needed  to  obtain  the  correct  solution.    Radiation  is  a 
condition. 
2.  The *CONTROL_THERMAL_NONLINEAR keyword is optional.  For example, the 
default values for remax (maximum number of iterations allowed per time step), tol 
(temperature  convergence tolerance),  and dcp  (divergence control tolerance) will be 
used,  if  the  nonlinear  keyword  is  omitted,  with  ptype>0  on  *CONTROL_
22.  1D Transient Heat Transfer in a Bar 
Keywords: 
*CONTROL_SOLUTION 
*CONTROL_THERMAL_SOLVER 
*CONTROL_THERMAL_TIMESTEP 
*BOUNDARY_TEMPERATURE_SET 
*INITIAL_TEMPERATURE_SET 
*MAT_THERMAL_ISOTROPIC 
Description: 
A  0.1  m  long  bar  (
yL )  cross-section  (Figure 
22.1),  is  subjected  at  one  end  (node  6)  to  a  varying  thermal  with  the  following  law: 
.    The  other  end  (node  1)  is  maintained  at  constant  temperature 
zL ),  with  square  0.01  m  (
xL )  x  0.01  m  (
100sin
/ 40

(
)
=
C= 
.  The bar is perfectly insulated along its length. 
Determine the temperature at 0.02 m from the hot end after 32 seconds. 
The bar is meshed with 20 elements: five elements along the length and four elements in 
the cross section.
Analysis Summary: 
Dim. 
Type 
Load  Material  Geometry  Contact 
Solver 
3D 
Thermal 
Transient 
Thermal  Linear 
Linear 
- 
Thermal 
Linear 
Solution 
Method 
3-Diagonal 
scaled 
conjugate 
gradient 
Units: 
kg, m, s, N, Pa, N-m,  C
degree Centigrade) - Joule (J) is a N-m, Watt (W) is a J/s 
 (kilogram, meter, second, Newton, Pascal, Newton-meter, 
Dimensional Data: 
xL
=
0.01
, 
yL
=
0.01
, 
zL
=
0.10
Material Data: 
Mass Density 
Heat Capacity 
Thermal Conductivity 
ρ=
pC
×
7.200 10
=
4.405 10
×
=
3.500 10
×
/kg m

/
J kg C

W m C
/
Load: 
Thermal 
Convection 
Initial Temperature 
Element Types: 
 (constant) 
W m C
/


=
100
×
=
7.500 10
C= 
 (all nodes) 
Fully integrated S/R solid (elform=2) 
Material Models:
Results Comparison: 
LS-DYNA  bar  temperature  at  x=0.0050  m,  y=0.005  m,  z=  0.080  m  (Node  35)  is 
compared with NAFEMS Background to Benchmark, Test T3. 
Reference Condition - Point Along Bar 
0.2 m (Node 35) from Hot End (Node 36) 
Temperature ( C
) 
NAFEMS Benchmark Test T3 
Node 35 
3.6600 10×
3.4861 10×
The  fully  integrated  selectively  reduced  solid  element  (elform=2)  model  (Figure  22.2) 
provides a reasonable temperature comparison for this coarse mesh. 
The problem is 1D, although done in 3D.  The results are, as expected, the same for all  
x-y planes along the Z-direction. 
Figure 22.2 -Contour plot of temperatures at time =32.0 seconds
The histories of temperature for two nodes (35 and 36) used in the comparison are shown 
in Figure 22.3. 
Figure 22.3 - Temperature histories for nodes 35 and 56. 
Input deck: 
*KEYWORD 
*TITLE 
1D Transient Heat Transfer in a Bar 
*CONTROL_SOLUTION 
$#    soln       nlq     isnan     lcint 
         1         0         0         0 
*CONTROL_THERMAL_SOLVER 
$#   atype     ptype    solver     cgtol       gpt    eqheat     fwork       sbc 
         1         0         3  1.00e-06         8  1.000000  1.000000       0.0 
*CONTROL_THERMAL_TIMESTEP 
$#      ts       tip       its      tmin      tmax     dtemp      tscp 
         1  0.500000 1.000e-04 1.000e-04  0.100000  1.000000  0.500000 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
  32.00000         0       0.0       0.0       0.0 
*DATABASE_TPRINT 
$#      dt    binary      lcur     ioopt 
  1.000000         0         0         1 
*DATABASE_HISTORY_NODE 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         5         6        11        12        17        18        23        24 
        29        30        35        36        41        42        47        48 
        53        54 
*DATABASE_BINARY_D3PLOT 
$#      dt      lcdt      beam     npltc    psetid 
  1.000000         0         0         0         0 
*PART 
$# title
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         0         0         0         0         0         1 
*SECTION_SOLID 
$#   secid    elform       aet 
         1         2         1 
*MAT_THERMAL_ISOTROPIC 
$#    tmid       tro     tgrlc    tgmult 
         1  7200.000       0.0       0.0 
$#      hc        tc 
  440.5000   35.0000 
*BOUNDARY_TEMPERATURE_SET 
$#    nsid      lcid     cmult       loc 
         1         0       0.0         0 
*BOUNDARY_TEMPERATURE_SET 
$#    nsid      lcid     cmult       loc 
         2         1  1.000000         0 
*INITIAL_TEMPERATURE_SET 
$#    nsid      temp       loc 
         3       0.0         0 
*SET_NODE_LIST_TITLE 
A 
$#     sid       da1       da2       da3       da4 
         1       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         1         7        13        19        25        31        37        43 
        49 
*SET_NODE_LIST_TITLE 
B  
$#     sid       da1       da2       da3       da4 
         2       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         6        12        18        24        30        36        42        48 
        54 
*SET_NODE_LIST_TITLE 
central 
$#     sid       da1       da2       da3       da4 
         3       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         1         2         3         4         5         6         7         8 
         9        10        11        12        13        14        15        16 
        17        18        19        20        21        22        23        24 
        25        26        27        28        29        30        31        32 
        33        34        35        36        37        38        39        40 
        41        42        43        44        45        46        47        48 
        49        50        51        52        53        54 
*DEFINE_CURVE 
$#    lcid      sdir       sfa       sfo      offa      offo     dattyp 
         1         0       0.0       0.0       0.0       0.0 
$#                a1                  o1 
                 0.0                 0.0 
          1.00000000          7.84194040 
          2.00000000         15.63558102 
          3.00000000         23.33292198 
          4.00000000         30.88655281 
          5.00000000         38.24995041 
          6.00000000         45.37776184 
          7.00000000         52.22608948 
          8.00000000         58.75275421 
          9.00000000         64.91754913 
         10.00000000         70.68251801 
         11.00000000         76.01214600 
         12.00000000         80.87360382 
         13.00000000         85.23696136 
         14.00000000         89.07533264 
         15.00000000         92.36508179 
         16.00000000         95.08594513 
         17.00000000         97.22116852 
         18.00000000         98.75759888 
         19.00000000         99.68576813 
         20.00000000         99.99996948
22.00000000         98.78250122 
         23.00000000         97.25833130 
         24.00000000         95.13513947 
         25.00000000         92.42600250 
         26.00000000         89.14760590 
         27.00000000         85.32013702 
         28.00000000         80.96717834 
         29.00000000         76.11553955 
         30.00000000         70.79508972 
         31.00000000         65.03861237 
         32.00000000         58.88155746 
*ELEMENT_SOLID 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       1      19      25       7       2      20      26       8 
      20       1      29      47      53      35      30      48      54      36 
*NODE 
$#   nid               x               y               z      tc      rc 
       1             0.0             0.0             0.0 
      54      0.01000000      0.01000000      0.10000000 
*END
23.  2D Heat Transfer with Convection 
Keywords: 
*CONTROL_SOLUTION 
*CONTROL_THERMAL_SOLVER 
*CONTROL_THERMAL_TIMESTEP 
*MAT_THERMAL_ISOTROPIC 
*BOUNDARY_CONVECTION_SET 
*BOUNDARY_TEMPERATURE_SET 
*INITIAL_TEMPERATURE_SET 
Description: 
=
=
xL
yL
1.00
 in depth) of rectangular cross-section (
A slab (
) 
shown  in  Figure  23.1  is  subjected  to  the  following  thermal  loads  for  a  steady  state 
simulation: 
•  constant Temperature 
0 =
•  natural  convection  to  the  ambient  temperature 
on the face defined by nodes 78-79-85-95, 
0=
nodes 12-85-79-18 and 1-12-18-2 (convection coefficient 
face defined by nodes 1-2-78-95 is adiabatically insulated. 
  on  the  faces  defined  by 
W m C
×
7.50 10
1.00
0.60
 by 
100
Ta
zL
), 
=
/
• 


=
Find the temperature at node 225 (x=0.60 m, y=1.00 m, z=-0.20 m).
Analysis Summary: 
Dim.  Type 
Load  Material  Geometry  Contact 
Solver 
Thermal  Linear 
Linear 
- 
Thermal 
3D 
Steady 
State 
Units: 
Solution 
Method 
3-Diagonal 
scaled 
conjugate 
gradient 
kg, m, s, N, Pa, N-m,  C
degree Centigrade) - Joule (J) is a N-m, Watt (W) is a J/s 
 (kilogram, meter, second, Newton, Pascal, Newton-meter, 
Dimensional Data: 
xL
=
0.60
, 
yL
=
1.00
, 
zL
=
1.00
Material Data: 
Mass Density 
Heat Capacity 
Thermal Conductivity 
ρ=
pC
=
×
8.000 10
=
1.000 10
×
5.200 10
×
/kg m

/
J kg C

W m C
/
Load: 
Thermal 
Convection 
Element Types: 
=
=

100
×
7.500 10
 (constant) 
W m C
/

Fully integrated S/R solid (elform=2) 
Material Models:
Results Comparison: 
LS-DYNA  slab  edge  temperature  at  x=0.60  m,  y=1.00  m,  z=-0.20  m  (Node  225)  are 
compared with NAFEMS Background to Benchmark, Test T4. 
Reference Condition - Point Along Slab 
Edge (Node 225) 
Temperature ( C
) 
NAFEMS Benchmark Test T4 
Node 225 
1.8300 10×
1.7954 10×
The  fully  integrated  selectively  reduced  solid  element  (elform=2)  model  (Figure  23.2) 
provides a reasonable temperature comparison for this relatively coarse mesh. 
The problem is 2D, although solved in 3D.  The results are, as expected, the same for all 
planes in the 3rd dimension (Y-direction in this case).
*TITLE 
2D Heat Transfer with Convection 
*CONTROL_SOLUTION 
$#    soln       nlq     isnan     lcint 
         1         0         0         0 
*CONTROL_THERMAL_SOLVER 
$#   atype     ptype    solver     cgtol       gpt    eqheat     fwork       sbc 
         0         0         3  1.00e-06         8  1.000000  1.000000  0.000000  
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
  1.000000         0     0.000     0.000     0.000 
*DATABASE_TPRINT 
$#      dt    binary      lcur     ioopt 
  1.000000         0         0         1 
*DATABASE_HISTORY_NODE 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
       225       171       371       372       373       374       375       376 
       377       378       379 
*DATABASE_BINARY_D3PLOT 
$#      dt      lcdt      beam     npltc    psetid 
  1.000000         0         0         0         0 
*PART 
$# title 
Part          1 for Mat         1 and Elem Type         2                        
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         0         0         0         0         0         1 
*SECTION_SOLID 
$#   secid    elform       aet 
         1         2         0 
*MAT_THERMAL_ISOTROPIC 
$#    tmid       tro     tgrlc    tgmult      tlat      hlat 
         1  8000.000     0.000     0.000     0.000     0.000 
$#      hc        tc 
     1.000   52.0000 
*BOUNDARY_CONVECTION_SET 
$#    ssid 
         1 
$#   hlcid     hmult     tlcid     tmult       loc 
         0 750.00000         0     0.000         0 
*BOUNDARY_CONVECTION_SET 
$#    ssid 
         2 
$#   hlcid     hmult     tlcid     tmult       loc 
         0 750.00000         0     0.000         0 
*BOUNDARY_TEMPERATURE_SET 
$#    nsid      lcid     cmult       loc 
         1         0 100.00000         0 
*INITIAL_TEMPERATURE_SET 
$#    nsid      temp       loc 
         1 100.00000         0 
*SET_NODE_LIST_TITLE 
frontt100 
$#     sid       da1       da2       da3       da4 
         1     0.000     0.000     0.000     0.000 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
        78        79        80        81        82        83        84        85 
        86        87        88        89        90        91        92        93 
        94        95        96        97        98        99       100       101 
       102       103       104       105       106       107       108       109 
       110       111       112       113       114       115       116       117 
       118       119       120       121       122       123       124       125 
       126       127       128       129       130       131       132       133 
       134       135       136       137       138       139       140       141 
       142       143       144       145       146       147       148       149 
       150       151       152       153       154         0         0         0 
*SET_SEGMENT_TITLE
$#     sid       da1       da2       da3       da4 
         1     0.000     0.000     0.000     0.000 
$#      n1        n2        n3        n4        a1        a2        a3        a4 
        18        19       434       164     0.000     0.000     0.000     0.000 
       370       226        85        94     0.000     0.000     0.000     0.000 
*SET_SEGMENT_TITLE 
backt0 
$#     sid       da1       da2       da3       da4 
         2     0.000     0.000     0.000     0.000 
$#      n1        n2        n3        n4        a1        a2        a3        a4 
         2        11        33        28     0.000     0.000     0.000     0.000 
        77        13        12        27     0.000     0.000     0.000     0.000 
*ELEMENT_SOLID 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       2      28      33      11     163     213     443     289 
     600       1     847     370     226     272     154      94      85      96 
*NODE 
$#   nid               x               y               z      tc      rc 
       1           0.000       1.0000000      -1.0000000       0       0 
     847       0.5000000       0.9000000      -0.1000000       0       0 
*END 
Notes: 
1.  A two-dimensional model simulation could be made using the plane stress (x-y plane) 
element  formulation  (elform=12  given  on  *SECTION_SHELL  keyword)  with  a 
constant  temperature  through  the  thickness.    Under  the  keyword  *CONTROL_ 
SHELL, the option  tshell  allows the user  to  choose  between  a  constant temperature 
through the thickness and a 20 node brick formulation which allows heat conduction
24.  3D Thermal Load 
Keywords: 
*CONTROL_IMPLICIT_GENERAL 
*CONTROL_IMPLICIT_SOLUTION 
*LOAD_THERMAL_VARIABLE_NODE 
*MAT_ELASTIC_PLASTIC_THERMAL 
Description: 
The  solid  cylinder  tapering  to  a  sphere  geometry  depicted  below  (Figure  24.1)  is 
subjected  to  a  prescribed  temperature  gradient.    Two  analyses,  one  with  a  coarse  mesh    
5  x  1  x  3  and  one  with  a  fine  mesh  10  x  2  x  3  (Figure  24.2),  are  made.    The  model 
represents  ¼  of  the  total  geometry.    Symmetry  conditions  on  the  plane  x-z  and  y-z  are 
enforced.  The faces parallel to the plane x-y are simply supported in the Z-direction. 
The  linear  temperature  loading  (radial  and  axial  direction)  (Figure  24.3)  is  applied  by 
means  of  temperature  dependent  material  with  thermal  expansion  coefficient  and 
resulting thermal strain 
Tαε =
. 
Determine  the  stress in the Z-direction at  Node  A (Node 10 for the coarse-mesh model 
and Node 16 for the fine-mesh model). 
Figure 24.1 - Schematic of ¼ model and cross-section dimensions
Figure 24.2 - Finite element models with selected node and element identified. 
Figure 24.3 - Finite element models with temperature loading. 
Analysis Summary: 
Dim.  Type 
Load  Material  Geometry  Contact 
Solver 
Solution 
Method 
3D 
Static 
Thermal  Linear 
Linear 
- 
Implicit 
1-Linear 
Units: 
kg, m, s, N, Pa, N-m,  C
degree Centigrade) - Joule (J) is a N-m, Watt (W) is a J/s 
 (kilogram, meter, second, Newton, Pascal, Newton-meter, 
Dimensional Data:
Material Data: 
Young's Modulus 
Poisson's Ratio 
Linear Expansion 
Load: 
Thermal 
Element Types: 
11
Pa
=
ν =
=
×
2.10 10
0.3
×
2.30 10
−
m m C
/
/


(
T C
)
=
+
+
Fully integrated S/R solid (elform=2) 
Material Models: 
*MAT_004 or *MAT_ELASTIC_PLASTIC_THERMAL 
Results Comparison: 
zzσ   at  inner  point  on  yz-symmetry  plane  (coarse  mesh  -  Node 
LS-DYNA  global  stress 
10, Element 3: fine mesh - Node 16, Element 5) is compared with NAFEMS Background 
to Benchmarks, Test LE11. 
Reference Condition - Inner 
Point on Symmetry Plane 
Coarse Mesh - Global 
Stress - 
zzσ  (MPa) 
Fine Mesh - Global 
zzσ  (MPa) 
Stress - 
NAFEMS Benchmark Test LE11 
Element 3 (coarse) - Element 5 
(fine) - (an averaged value) 
First in-plane integration point - 
Elem 3 (coarse) - Element 5 (fine) 
Node 10 (coarse) - Node 16 (fine) 
−
1.0500 10
×
−
1.0500 10
×
−
6.1849 10
×
−
7.5890 10
×
−
7.9107 10
×
−
8.5217 10
×
−
9.2071 10
×
−
9.2102 10
×
zzσ  results were generated from *DATABASE_ELOUT (elout file) and 
The global stress 
*DATABASE_EXTENT_BINARY  (eloutdet  file  provides  detailed  element  output  at
By  default,  stresses/strains  for  solids  are  written  to  d3plot  and  elout  in  the  global 
coordinate  system.    The  elout  file  contains  only  the  values  at  the  element  centroid 
(average of 8 integration points). 
You  can  set  intout=stress  or  intout=all  (*DATABASE_EXTENT_BINARY)  and  have 
stresses  output 
file  called  eloutdet 
integration  points 
(*DATABASE_ELOUT  governs  the  output  interval  and  *DATABASE_HISTORY_ 
SOLID  governs  which  elements  are  output).    Setting  nodout=stress  or  nodout=all  in 
*DATABASE_EXTENT_BINARY will write the extrapolated nodal stresses to eloutdet. 
for  all 
to  a 
the 
LS-DYNA stress and strain outputs correspond to integration point locations.  Stress at a 
node  is  an  artifact  of  the  post-processor  and  represents  an  average  of  the  surrounding 
integration point stresses (the value will likely be different with different postprocessors). 
zzσ  at 
Both meshes are rather coarse which makes it difficult to capture the global stress 
the inner point along yz-symmetry plane.  The extrapolated nodal stress results (also see 
Figures  24.4  and  24.5)  provide  the  best  comparative  value  (~12%  difference  for  both 
meshes), primarily  due to the nodal location.    As expected,  the  fine mesh does a  better 
job  of  capturing  the  overall  contouring.    The  average  global  stress  of  the  element 
provides  the  least  acceptable  comparative  value  results  (~40%  and  ~25%  differences), 
again  not  unexpected,  while  the  nearest  element  integration  point  results  provided 
significant  improvement  (~25%  and  ~15%  differences)  due  to  the  larger  integration 
sample (8 points as compared to 1) and nodal location. 
Figure 24.4 - Coarse mesh contour plots of global stress σzz  with average value given 
for Element 3.  On the left is in-plane integration point contouring while on the right
Figure 24.5 - Fine mesh contour plots of global stress σzz  with average value given 
for Element 5.  On the left is in-plane integration point contouring while on the right 
is extrapolated nodal stress contouring with specification values given at Node 16. 
Input deck: 
*KEYWORD 
*TITLE 
3D Thermal Load (coarse mesh) 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form 
         1  1.000000         2         1         2 
*CONTROL_IMPLICIT_SOLUTION 
$#  nsolvr    ilimit    maxref     dctol     ectol     rctol     lstol    abstol 
         1        11        15  0.001000  0.010000   1.0e+10  0.900000  1.000000 
$#   dnorm    diverg     istif   nlprint    nlnorm    d3itcl     cpchk 
         2         1         1         2         2         0         0 
$#  arcctl    arcdir    arclen    arcmth    arcdmp    arcpsi    arcalf    arctim 
         0         1       0.0         1         2       0.0       0.0       0.0 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
  1.000000         0       0.0       0.0       0.0 
*DATABASE_EXTENT_BINARY 
$#   neiph     neips    maxint    strflg    sigflg    epsflg     rtflg    engflg 
         0         0         0         1         1         1         1         1 
$#  cmpflg    ieverp    beamip     dcomp      shge     stssz    n3thdt   ialemat 
$# nintsld   pkp_sen      sclp     hydro     msscl     therm    intout    nodout 
         8                 1.0                                  stress    stress 
*DATABASE_ELOUT 
$# dt/cycl 
  0.100000 
*DATABASE_HISTORY_SOLID 
$#    eid1      eid2      eid3      eid4       ei5      eid6      eid7      eid8 
         3 
*DATABASE_BINARY_D3PLOT 
$# dt/cycl 
  1.000000 
*PART 
$# title                                                                         
Part          1 for Mat         1 and Elem Type          2                       
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1 
*SECTION_SOLID 
$#   secid    elform       aet 
         1         2         1 
*MAT_ELASTIC_PLASTIC_THERMAL 
$#     mid        ro 
         1  1.000000
0.0  1000.000       0.0       0.0       0.0       0.0       0.0       0.0 
$#      e1        e2        e3        e4        e5        e6        e7        e8 
 2.100e+11 2.100e+11       0.0       0.0       0.0       0.0       0.0       0.0 
$#     pr1       pr2       pr3       pr4       pr5       pr6       pr7       pr8 
  0.300000  0.300000       0.0       0.0       0.0       0.0       0.0       0.0 
$#  alpha1    alpha2    alpha3    alpha4    alpha5    alpha6    alpha7    alpha8 
 2.300e-04 2.300e-04       0.0       0.0       0.0       0.0       0.0       0.0 
$#   sigy1     sigy2     sigy3     sigy4     sigy5     sigy6     sigy7     sigy8 
       0.0       0.0       0.0       0.0       0.0       0.0       0.0       0.0 
$#   etan1     etan2     etan3     etan4     etan5     etan6     etan7     etan8 
       0.0       0.0       0.0       0.0       0.0       0.0       0.0       0.0 
*ELEMENT_SOLID 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       1      13      16       4       2      14      17       5 
      15       1      35      39      40      36      43      47      48      44 
*NODE 
$#   nid               x               y               z      tc      rc 
       1       1.0000000           0.000           0.000       0       0 
      48           0.000       1.0000000       1.7900000       0       0 
*SET_NODE_LIST_TITLE 
base 
$#     sid       da1       da2       da3       da4    solver 
         1       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
        19         7         4        16 
*SET_NODE_LIST_TITLE 
top 
$#     sid       da1       da2       da3       da4    solver 
         2       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
        43        47        46        42 
*SET_NODE_LIST_TITLE 
xsymm 
$#     sid       da1       da2       da3       da4    solver 
         3       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
        23        11        24        12        28        32        40        36 
*SET_NODE_LIST_TITLE 
ysymm 
$#     sid       da1       da2       da3       da4    solver 
         4       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         2        14         3        15        25        29        33        37 
*SET_NODE_LIST_TITLE 
z+ysymm 
$#     sid       da1       da2       da3       da4    solver 
         5       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         1        13        41        45 
*SET_NODE_LIST_TITLE 
z+xsymm 
$#     sid       da1       da2       da3       da4    solver 
         6       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
        22        10        48        44 
*BOUNDARY_SPC_SET 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         1         0         0         0         1 
*BOUNDARY_SPC_SET 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         2         0         0         0         1 
*BOUNDARY_SPC_SET 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         3         0         1         0         0 
*BOUNDARY_SPC_SET 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         4         0         0         1         0 
*BOUNDARY_SPC_SET
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         6         0         1         0         1 
*LOAD_THERMAL_VARIABLE_NODE 
$#     nid        ts        tb      lcid 
         1  1.000000       0.0         1 
        48  2.790000       0.0         1 
*DEFINE_CURVE 
$#    lcid      sdir       sfa       sfo      offa      offo     dattyp 
         1         0       0.0       0.0       0.0       0.0 
$#                a1                  o1 
                 0.0          1.00000000 
          1.00000000          1.00000000 
*END 
Notes: 
1.  The fully integrated solid elements are formulated for nonlinear analysis.  Although 
this  analysis  is  linear,  it  could  have  been  solved  with  a  nonlinear  solution  method 
(nsolvr=2).  This was done for this simulation and it was found to yield results with 
some differences (less than 0.01% for coarse mesh and ~4% for fine mesh) from the 
linear  analysis  (nsolvr=1).    It  is  not  understood  why  the  fine  mesh  offers  this 
difference. 
2.  Fully-integrated  solid  formulations  have  8  in-volume  integration  points  for  each 
element.  For these formulations, the 8 values of each stress component are averaged 
at the element centroid before being written to elout. 
3.  If  setting  nintsld=8  on  *DATABASE_EXTENT_BINARY,  LS-DYNA  will  write 
stresses  at  all  integration  points  for  solid  elements  (also  given  in  eloutdet)  to  the 
d3plot file.  When this option is set, LS-PrePost applies the stress values to the nodes 
from  the  closest  integration  point  and  after  that,  the  average  value  from  the 
contributions are computed and presented in the stress fringe plot. 
4.  A  command  line  option  (extrapolate  1)  is  added  to  LS-PrePost,  which  will  linearly 
extrapolate  the  values  from  integration  points  to  the  nodes  (the  extrapolated  nodal 
stresses are also given in eloutdet). 
5.  For  elastic  bending,  two  integrations  points  through  the  thickness  is  the  minimum 
number.    For  plastic  bending,  three  integrations  points  through  the  thickness  is  the
25.  Cooling of a Billet via Radiation 
Keywords: 
*CONTROL_SOLUTION 
*CONTROL_THERMAL_SOLVER 
*CONTROL_THERMAL_NONLINEAR 
*CONTROL_THERMAL_TIMESTEP 
*BOUNDARY_TEMPERATURE_SET 
*BOUNDARY_RADIATION_SET 
*MAT_THERMAL_ISOTROPIC 
Description: 
=
=
ft
4.00
2.00
A  billet  (
zL
) shown in Figure 25.1 is initially at temperature 
ft
  in  height)  of  rectangular  cross-section  (
 loses heat by 
radiation  (transient)  from  all  its  surfaces  to  its  surroundings  at  a  temperature  of 
eT
.  There is zero internal heat generation. 
=
2.00
ft
  by 
xL

2000
530
=
=

Determine the temperature of the billet (e.g. Node 625) after 3.7 hours (
×
1.3320 10 sec
). 
The bar is meshed with 432 elements: 12 elements along the height and 36 elements in 
the cross section.
Analysis Summary: 
Dim. 
Type 
Load  Material  Geometry  Contact 
Solver 
3D 
Thermal 
Transient  Thermal  Linear 
Linear 
- 
Thermal 
Nonlinear 
Solution 
Method 
3-Diagonal 
scaled 
conjugate 
gradient 
Units: 
lbf-s2/ft, ft, s, lbf, psf, lbf-ft (slug, foot, second, pound force, pound force/foot2, 

pound force-foot) - Thermal Energy is a Btu, Power is a Btu/s, 1

∆ = ∆
1F
Dimensional Data: 
xL
=
2.00
ft
, 
yL
=
2.00
ft
, 
zL
=
2.00
ft
Material Data: 
Mass Density 
Heat Capacity 
×
4.875 10
=
1.100 10
×
lbf
−
−
/
/
Btu lbf
−
Btu ft
/
ft
−
 (arbitrary value) 
ρ=
pC
=
ε=
Thermal Conductivity 
Emissivity 
×
1.000 10
1.000
Stefan-Boltzman 
=
4.750 10
×
−
13
/Btu s
−
ft
−
Load: 
Thermal (billet) 
Thermal (outside) 
eT
=
=
Element Types: 
2000.0

530.0

 (constant) 
 (surroundings) 
Fully integrated S/R solid (elform=2) 
Material Models:
Results Comparison: 
LS-DYNA temperature of the billet at selected point x=2.000 ft, y=2.010 ft, z= 0.000 ft 
(Node  625)  is  compared  with  R.  Siegal  and  J.R.  Howell  studies  in  Thermal  Radiation 
Heat Transfer, 1981, pg. 229. 
Reference Condition - Billet 
Temperature ( R
) at t=13320 sec 
Siegal and Howell [1981] 
Node 625 
1.0000 10×
1.0080 10×
The  fully  integrated  selectively  reduced  solid  element  (elform=2)  model  provides  a 
reasonable temperature comparison for this mesh (less that 1% difference). 
With  the  given  simple  geometry  plus  the  initial  temperature  and  radiation  heat  losses 
being space invariant, the temperature is uniform throughout the mesh. 
The temperature history of Node 625 used in the comparison is shown in Figure 25.2.
*TITLE 
Cooling of a Billet Via Radiation 
*CONTROL_SOLUTION 
$#    soln       nlq     isnan     lcint 
         1         0         0         0 
*CONTROL_THERMAL_SOLVER 
$#   atype     ptype    solver     cgtol       gpt    eqheat     fwork       sbc 
         1         2         3  1.00e-06         1  1.000000  1.0000004.7500e-13 
*CONTROL_THERMAL_NONLINEAR 
$#  refmax       tol       dcp 
        20 1.000e-06  0.500000 
*CONTROL_THERMAL_TIMESTEP 
$#      ts       tip       its      tmin      tmax     dtemp      tscp 
         1  0.500000  0.100000  0.100000  100.0000  1.000000  0.500000 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
1.3320e+04         0       0.0       0.0       0.0 
*DATABASE_TPRINT 
$#      dt    binary      lcur     ioopt 
  10.00000         0         0         1 
*DATABASE_HISTORY_NODE 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         1        13        79       265 
*DATABASE_BINARY_D3PLOT 
$#      dt      lcdt      beam     npltc    psetid 
  100.0000         0         0         0         0 
*PART 
$# title                                                                         
Part          1 for TMat        1 and Elem Type         2                        
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         0         0         0         0         0         1 
*SECTION_SOLID 
$#   secid    elform       aet 
         1         2         1 
*MAT_THERMAL_ISOTROPIC 
$#    tmid       tro     tgrlc    tgmult 
         1  487.5000       0.0       0.0 
$#      hc        tc 
   0.11000 1.000e+04 
*BOUNDARY_RADIATION_SET 
$#    ssid      type 
         1         1 
$#   flcid     fmult    tilcid    timult       loc 
         04.7500e-13         0  530.0000         0 
*INITIAL_TEMPERATURE_SET 
$#    nsid      temp       loc 
         1 2000.0000         0 
*SET_NODE_LIST_TITLE 
all 
$#     sid       da1       da2       da3       da4 
         1       0.0       0.0       0.0       0.0 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         1         2         3         4         5         6         7         8 
       633       634       635       636       637 
*SET_SEGMENT_TITLE 
rad_surf 
$#     sid       da1       da2       da3       da4 
         1       0.0       0.0       0.0       0.0 
$#      n1        n2        n3        n4        a1        a2        a3        a4 
        92        93         2         1       0.0       0.0       0.0       0.0 
       545       546       637       636       0.0       0.0       0.0       0.0 
*ELEMENT_SOLID 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8
$#   nid               x               y               z      tc      rc 
       1             0.0             0.0             0.0 
     637      2.00000000      2.00000000      4.00000000 
*END 
Notes: 
1.  The problem must be flagged as nonlinear if any boundary  condition parameter is a 
function  of  temperature  T.    This  includes  a  linear  (i.e.,  straight  line)  relationship.  
4T  temperature 
Iterations are needed to obtain the correct solution.  Radiation (q) is a 
boundary condition (usually F=1): 
=
σε
F T
(
surface
−
∞
)
2.  The *CONTROL_THERMAL_NONLINEAR keyword is optional.  For example, the 
default values for remax (maximum number of iterations allowed per time step), tol 
(temperature  convergence tolerance),  and dcp  (divergence control tolerance) will be 
used,  if  the  nonlinear  keyword  is  omitted,  with  ptype>0  on  *CONTROL_ 
THERMAL_SOLUTION keyword. 
3.  This  study  could  have  been  performed  using  a  single  element  with  the  following 
modifications to the above input deck: 
*SET_NODE_LIST_TITLE 
all 
         1       0.0       0.0       0.0       0.0 
         1         2         3         4         5         6         7         8 
*SET_SEGMENT_TITLE 
ext_surf 
$#     sid       da1       da2       da3       da4 
         1       0.0       0.0       0.0       0.0 
$#      n1        n2        n3        n4        a1        a2        a3        a4 
         2         3         7         6       0.0       0.0       0.0       0.0 
         7         8         5         6       0.0       0.0       0.0       0.0 
         4         8         7         3       0.0       0.0       0.0       0.0 
         2         6         5         1       0.0       0.0       0.0       0.0 
         4         1         5         8       0.0       0.0       0.0       0.0 
         1         4         3         2       0.0       0.0       0.0       0.0 
*ELEMENT_SOLID 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       1       2       3       4       5       6       7       8 
*NODE 
       1             0.0             0.0             0.0 
       2      2.00000000             0.0             0.0 
       3      2.00000000      2.00000000             0.0 
       4             0.0      2.00000000             0.0 
       5             0.0             0.0      4.00000000 
       6      2.00000000             0.0      4.00000000 
       7      2.00000000      2.00000000      4.00000000 
       8             0.0      2.00000000      4.00000000 
This  single  element  representation  provides  the  identical  temperature  result  at  t=3.7 
hours (
) as the 432 element mesh. 
×
1.3320 10 sec
26.  Pipe Whip 
Keywords: 
*CONTROL_CONTACT 
*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_TITLE 
*MAT_PLASTIC_KINEMATIC 
*MAT_RIGID 
*INITIAL_VELOCITY_GENERATION 
*CONSTRAINED_EXTRA_NODES_SET 
Description: 
This problem illustrates the capabilities of LS-DYNA in a high speed, large deformation 
event with complex contact conditions, e.g. a pipe-on-pipe impact. 
The pipes are modeled using fully integrated shell elements. 
The impacted pipe is fully restrained, translationally and rotationally, at both ends (
and 
initial angular speed of 75 rad/s about a fixed point at one end (Figures 26.1 and 26.2). 
x =  
= ),  while the impacting pipe is rotating at an 
x L=
: 
=
=
=
=
=
The pipe material is elastic-perfectly plastic, and the material model *MAT_PLASTIC_ 
KINEMATIC with zero tangent modulus is appropriate. 
The initial rotational velocity is imposed through the keyword *INITIAL_VELOCITY_ 
GENERATION.  A rigid, rotational end joint is defined using the pipe's end ring of nodes 
which  are  made  rigid  using 
the  *CONSTRAINED_EXTRA_NODES_SET  and 
*MAT_RIGID keywords. 
The  contact  is  *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE.    This  contact 
has the following characteristics: 
• 
it is a two-way contact, in that user-specified slave nodes are checked for penetration 
of  the  master  segments  and  then  a  second  time,  to  check  the  master-side  nodes  for 
penetration through the slave segments, 
the  treatment  is  thus  symmetric  and  the  definition  of  the  slave  surface  and  master 
surface is arbitrary, 
• 
•  AUTOMATIC contacts check for penetration on either side of a shell element, 
• 
this  is  a  recommended  contact  type  in  large  deformation  application,  e.g.  in  crash 
simulations,  since  the  orientation  of  parts  relative  to  each  other  cannot  always  be 
anticipated. 
Shell  thickness  is  considered  with  option  shlthk=1.    The  soft=2  option  (segment  based
Figure 26.1 – Finite element model with boundary condition nodes (marked 
with 's ).  There are100 elements axially and 40 elements circumferentially. 
Figure 26.2 – Half-symmetry finite element model of a 50 in
Analysis Summary: 
Dim. 
Type 
Load  Material  Geometry  Contact 
Solver 
Solution 
Method 
3D  Dynamic  Velocity 
Non-
linear 
Linear 
3D 
Explicit 
Units: 
lbf-s2/in, in, s, lbf, psi, lbf-in (blob, inch, second, pound force, pound force/inch2, 
pound force-inch) 
Dimensional Data: 
=
=
5.000 10
×
in
, 
=
4.320 10
×
in−
Material Data: 
Mass Density 
Young's Modulus 
Poisson's Ratio 
Yield Stress 
Tangent Modulus 
Load: 
Velocity 
Element Types: 
=
7.324 10
×
−
lbf
−
/
in
lbf
/
in
lbf
/
in
×
3.000 10
0.3
4.500 10
×
=
ν =
σ =
tE
=
0.000 10
×
lbf
/
in
ω=
7.500 10
×
rad s
/
Fully integrated shell (elform=16) 
Material Models: 
*MAT_003 or *MAT_PLASTIC_KINEMATIC
Results Comparison: 
The results for deformed shapes taken from R.M. Ferencz studies on Element-by-Element 
Preconditioning  Techniques  for  Large-Scale,  Vectorized  Finite  Element  Analysis  in 
Nonlinear Solid and Structural Mechanic, March, 1989 (pg. 142) are reproduced here in 
Figure  26.3.    The  LS-DYNA  results  for  deformed  shapes  at  selected  times  in  the 
simulation (Figures 26.4a and 26.4b) are in good agreement.
Figure 26.4a – Half-symmetry deformed shapes at 0.0025, 
0.0050, 0.0100, and 0.0150 sec (hidden line view). 
Figure 26.4b – Half-symmetry deformed shapes at 0.0025,
The histories of the kinetic energy, internal energy, sliding energy, and the total energy 
are given in Figure 26.5. 
Nearly  all  of  the  initial  kinetic  energy  has  been  converted  into  plastic  deformation 
(internal energy) due to the pipe deformation. 
There is a small amount of energy dissipated in the contact (sliding energy) between the 
pipes, which, when included in the output computation, makes for an energy balance. 
Figure 26.5 – Histories of the kinetic energy, internal 
energy, sliding energy, and the total energy. 
Input Deck: 
*KEYWORD 
*TITLE 
Pipe Whip 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
  0.015000         0       0.0       0.0       0.0 
*CONTROL_TIMESTEP 
$#  dtinit    tssfac      isdo    tslimt     dt2ms      lctm     erode     ms1st 
       0.0  0.900000 
$#  dt2msf   dt2mslc     imscl 
       0.0         0         0 
*CONTROL_CONTACT 
$#  slsfac    rwpnal    islchk    shlthk    penopt    thkchg     orien    enmass 
  1.000000       0.0         2         2         0         0         1
0         0         0         0  4.000000 
$#   sfric     dfric       edc       vfc        th     th_sf    pen_sf 
       0.0       0.0       0.0       0.0       0.0       0.0       0.0 
$#  ignore    frceng   skiprwg 
         0         0         0 
*CONTROL_ENERGY 
$#    hgen      rwen    slnten     rylen 
         2         2         2         2 
*DATABASE_GLSTAT 
$#      dt    binary 
1.0000e-05         1 
*DATABASE_MATSUM 
$#      dt    binary 
1.0000e-05         1 
$#      dt    binary 
*DATABASE_SLEOUT 
1.0000e-05         1 
*DATABASE_BINARY_D3PLOT 
$# dt/cycl   lcdt/nr      beam     npltc    psetid 
2.5000e-04 
*PART 
$# title                                                                         
material type # 3 (Kinematic/Isotropic Elastic-Plastic)                          
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1         0         1 
*SECTION_SHELL 
$#   secid    elform      shrf       nip     propt   qr/irid     icomp     setyp 
         1        16   0.83333       5.0         1       0.0         0         1 
$#      t1        t2        t3        t4      nloc     marea 
  0.432000  0.432000  0.432000  0.432000         0       0.0 
*MAT_PLASTIC_KINEMATIC 
$#     mid        ro         e        pr      sigy      etan      beta 
         1 7.324e-04 3.000e+07  0.300000 4.500e+04       0.0       0.0 
$#     src       srp        fs        vp 
       0.0       0.0       0.0       0.0 
*HOURGLASS 
$#    hgid       ihq        qm       ibq        q1        q2        qb        qw 
         1         0       0.0         0       0.0       0.0       0.0       0.0 
*PART 
$# title                                                                         
material type # 3 (Kinematic/Isotropic Elastic-Plastic)                          
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         2         2         2         0         2         0         1 
*SECTION_SHELL 
$#   secid    elform      shrf       nip     propt   qr/irid     icomp     setyp 
         2        16   0.83333       5.0         1       0.0         0         1 
$#      t1        t2        t3        t4      nloc     marea 
  0.432000  0.432000  0.432000  0.432000         0       0.0 
*MAT_PLASTIC_KINEMATIC 
$#     mid        ro         e        pr      sigy      etan      beta 
         2 7.324e-04 3.000e+07  0.300000 4.500e+04       0.0       0.0 
$#     src       srp        fs        vp 
       0.0       0.0       0.0       0.0 
*HOURGLASS 
$#    hgid       ihq        qm       ibq        q1        q2        qb        qw 
         2         0       0.0         0       0.0       0.0       0.0       0.0 
*PART 
$# title                                                                         
material type # 20 (Rigid)                                                       
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
        99        99        99 
*SECTION_SHELL 
$#   secid    elform      shrf       nip     propt   qr/irid     icomp     setyp 
        99         2   0.83333       1.0         1       0.0         0         1 
$#      t1        t2        t3        t4      nloc     marea 
  0.432000  0.432000  0.432000  0.432000         0       0.0 
*MAT_RIGID 
$#     mid        ro         e        pr         n    couple         m     alias 
        99 7.324e-04 3.000e+07  0.300000       0.0       0.0       0.0 
$#     cmo      con1      con2
$#lco or a1       a2        a3        v1        v2        v3 
       0.0       0.0       0.0       0.0       0.0       0.0 
*CONSTRAINED_EXTRA_NODES_SET 
$#     pid      nsid 
        99        99 
*SET_NODE_LIST_TITLE 
rigid ring of nodes 
$#     sid       da1       da2       da3       da4    solver 
        99     0.000     0.000     0.000     0.000MECH 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
      8041      8042      8043      8044      8045      8046      8047      8048 
      8049      8050      8051      8052      8053      8054      8055      8056 
      8057      8058      8059      8060      8061      8062      8063      8064 
      8065      8066      8067      8068      8069      8070      8071      8072 
      8073      8074      8075      8076      8077      8078      8079      8080 
*INITIAL_VELOCITY_GENERATION 
$#      id      styp     omega        vx        vy        vz     ivatn      icid 
         2         2    75.000       0.0       0.0       0.0         0         0 
$#      xc        yc        zc        nx        ny        nz     phase    irigid 
 25.000000 50.000000  6.725000  1.000000       0.0       0.0         0         0 
*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_TITLE 
$#     cid                                                                 title 
         1 
$#    ssid      msid     sstyp     mstyp    sboxid    mboxid       spr       mpr 
         1         2         3         3         0         0         0         0 
$#      fs        fd        dc        vc       vdc    penchk        bt        dt 
       0.0       0.0       0.0       0.0       0.0         0       0.0       0.0 
$#     sfs       sfm       sst       mst      sfst      sfmt       fsf       vsf 
       0.0       0.0       0.0       0.0       0.0       0.0       0.0       0.0 
$#    soft    sofscl    lcidab    maxpar     sbopt     depth     bsort    frcfrq 
         2  0.100000         0     1.025       0.0         2        10         1 
$#  penmax    thkopt    shlthk     snlog      isym     i2d3d    sldthk    sldstf 
       0.0         0         1         0         0         0       0.0       0.0 
$#    igap    ignore 
         2         0 
*ELEMENT_SHELL 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       1       2      42      41       0       0       0       0 
    8000       2    8040    8001    8041    8080       0       0       0       0 
*NODE 
$#   nid               x               y               z      tc      rc 
       1           0.000       28.096500           0.000       0       0 
    8080       28.058376       50.000000        7.209399       0       0 
*SET_NODE_LIST 
$#     sid       da1       da2       da3       da4    solver 
         1     0.000     0.000     0.000     0.000MECH 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
         1         2         3         4         5         6         7         8 
         9        10        11        12        13        14        15        16 
        17        18        19        20        21        22        23        24 
        25        26        27        28        29        30        31        32 
        33        34        35        36        37        38        39        40 
*SET_NODE_LIST 
$#     sid       da1       da2       da3       da4    solver 
         2     0.000     0.000     0.000     0.000MECH 
$#    nid1      nid2      nid3      nid4      nid5      nid6      nid7      nid8 
      4001      4002      4003      4004      4005      4006      4007      4008 
      4009      4010      4011      4012      4013      4014      4015      4016 
      4017      4018      4019      4020      4021      4022      4023      4024 
      4025      4026      4027      4028      4029      4030      4031      4032 
      4033      4034      4035      4036      4037      4038      4039      4040 
*BOUNDARY_SPC_SET 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         1         0         1         1         1         1         1         1 
*BOUNDARY_SPC_SET 
$#nid/nsid       cid      dofx      dofy      dofz     dofrx     dofry     dofrz 
         2         0         1         1         1         1         1         1
Notes: 
1.  The  general  contact  *CONTACT_AUTOMATIC_SINGLE_SURFACE  could  also 
have been used.  This type of contact has the following characteristics: 
•  a single contact surface is created for all the parts included in the contact, 
•  self contact is considered, 
• 
it is robust, reliable and accurate, making it the ideal choice  for crashworthiness 
and impact applications. 
By default, if ssid (slave segment id) is zero or blank, all part IDs are included in the 
contact.  A *PART_SET entry can be used to reduce the size of the part list. 
2.  The  most  common  contact-related  output  file,  rcforc,  is  produced  by  including  a 
*DATABASE_RCFORC  keyword  in  the  input  deck.    rcforc  is  an  ASCII  file 
containing  resultant  contact  forces  for  the  slave  and  master  sides  of  each  contact 
interface.  The forces are provided in the global coordinate system.  Note that rcforc 
data  is  not  provided  for  single  surface  contacts  as  all  the  contact  forces  from  this 
contact  type  come  from  the  slave  side  (as  there  is  no  master  side)  and  thus  the  net 
contact forces are zero.  To obtain rcforc data when single surface contacts are used, 
one  or  more  force  transducers  should  be  added  via  the  *CONTACT_FORCE_ 
TRANSDUCER_PENALTY keyword.  A force transducer simply measures contact 
forces produced by other contact interfaces defined in the model. 
3.  By  including  a  *DATABASE_SLEOUT  keyword,  individual  contact  interface 
energies  are  written  to  the  ASCII  output  file  sleout.    The  global  contact  energy  is
27.  Copper Bar Impacting a Rigid Wall 
Keywords: 
*CONTROL_ALE 
*CONTROL_CONTACT 
*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE 
*RIGIDWALL_PLANAR 
*INITIAL_VELOCITY_GENERATION 
*SECTION_SOLID 
*HOURGLASS 
Description: 
This problem is known in the literature as "Taylor Bar Impact Test" and is used to assess 
material  properties  (plastic  flow)  under  dynamic  conditions.    A  deformable  copper  bar 
impacts a rigid wall at high speed.  The deformed length (shortening), spread (widening), 
and maximum effective plastic strain (εp ) of the bar is determined. 
The  contact  of  the  deformable  body  and  the  rigid  wall  can  be  modeled  in  one  of  the 
following ways: 
• 
rigid  wall  (*RIGIDWALL_PLANAR),  which  provides  an  easy  way  to  treat  contact 
between a rigid-flat surface and the nodes of a deformable body, 
•  using geometric entities (*CONTACT_ENTITY), 
•  using a wall modeled with rigid shell elements  and a *CONTACT_AUTOMATIC_ 
SURFACE_TO_SURFACE. 
Two  of  these  methods  are  demonstrated  for  rigid  wall  contact,  (1)  the  rigid  wall  is 
modeled  with  rigid  shell  elements  (penalty  method)  and  (2)  the  wall  is  modeled  as  a 
planar rigid boundary.  The latter uses a constraint method which represents a perfectly 
plastic impact since, once penetration into the rigid wall is detected, the acceleration and 
velocity of the nodes are set to zero.  No friction is included. 
The  material  is  elastic-plastic  with  constant  tangent  stiffness  and  the  material  model 
*MAT_PLASTIC_KINEMATIC is used. 
For  comparison,  different  solid  hexahedron  (elform=1,2,-2,-1)  and 
tetrahedron 
(elform=10,13) elements, are used to model the bar as shown in Figure 27.1.  Hourglass 
control  is  used  with  the  default  value  (ihq=2  -  Flanagan-Belytschko  viscous  form  with 
coefficient qm=0.10) for the one-point quadrature element formulations. 
Traditional  Lagrangian  approaches,  for  large  deformations,  often  result  in  highly 
distorted  meshes  for  the  elements  close  to  the  impacted  region,  leading  to  loss  of 
accuracy  and  decreasing  the  critical  time  step  for  the  simulation.    Therefore,  a  simple 
Arbitrary Lagrangian-Eulerian (ALE) formulation (elform=5) is also presented.  A mix of 
simple average smoothing and volume weighted smoothing is used for the interior nodal
The (elform=5) formulation is single material ALE with Lagrange outer boundary node 
treatment  and  mesh  smoothing  effective  for  only  moderate  deformation.    Thus 
application of this formulation is limited to mostly academic problems, since there are not 
many practical applications for use of this feature.  In fact, this "Taylor Bar Impact Test" 
may be the only known practical application. 
Figure 27.1 – Finite element models of the impacting bar using hexahedron and 
tetrahedron elements (shell elements were used to model the impacted rigid plate).  
Each of these solid element meshes has 36 elements axially.  There are 288 and 1440 
elements per row for the hexahedron and tetrahedron models, respectively. 
Analysis Summary: 
Dim. 
Type 
Load  Material  Geometry  Contact 
Solver 
3D  Dynamic  Velocity 
Non-
linear 
Non-
linear 
3D 
Explicit 
Solution 
Method 
Lagrangian 
and ALE 
Units: 
g, mm, ms, N, MPa, N-mm (gram, millimeter, millisecond, Newton, MegaPascal, Newton-
Dimensional Data: 
=
3.240 10
×
mm
, 
=
6.400 10
×
mm
Material Data: 
Mass Density 
=
−
×
×
8.930 10
1.170 10
0.35
4.000 10
×
/g mm
MPa
MPa
1.000 10
×
MPa
=
ν =
σ =
tE
=
zV
=
2.270 10
×
mm ms
/
Young's Modulus 
Poisson's Ratio 
Yield Stress 
Tangent Modulus 
Load: 
Velocity 
Element Types: 
Constant stress solid (elform=1) 
Fully integrated S/R solid (elform=2) 
Fully integrated S/R solid - for poor aspect ratio (acc) - (elform=-2) 
Fully integrated S/R solid - for poor aspect ratio (eff) - (elform=-1) 
1 point tetrahedron (elform=10) 
1 point nodal pressure tetrahedron (elform=13) 
1 point ALE (elform=5) 
Material Models: 
*MAT_003 or *MAT_PLASTIC_KINEMATIC 
*MAT_020 or *MAT_RIGID 
Results Comparison: 
The  results  for  deformed  shapes  at  0.0,  5,  20,  and  80  ms,  taken  from  R.M.  Ferencz 
studies on Element-by-Element  Preconditioning Techniques for Large-Scale, Vectorized 
Finite Element Analysis in Nonlinear Solid and Structural Mechanics, March, 1989 (pg. 
86), are reproduced here in Figure 27.2.  Ferencz [1989] used NIKE3D  and its implicit 
dynamics solver.  The LS-DYNA results for deformed shapes at 80.0 ms (Figures 27.3a 
to  27.3g)  using  penalty  method  contact  and  rigid  boundary  contact  (Figures  27.7a  to 
) given 
27.7g) are in good agreement.  The maximum effective plastic strain (
by  Ferencz  [1989]  differs  significantly  from  the  non-ALE  results  of  LS-DYNA 
2.248
2.9
ε ≅p
(
from the highly distorted elements in the vicinity of the rigid wall. 
),  even  though  both  use  a  Lagrangian  approach;  these  values  are  taken 
3.9
to
Figure 27.2 – Deformed shapes (Ferencz [1989]) at 0.0, 5, 20, and 80 ms. 
Penalty Method 
(Rigid Mesh Material) 
Shortening 
(mm) 
Widening 
(mm) 
Max. plastic 
strain (εp ) 
Normalized 
CPU Time 
Constant stress solid 
(elform=1) 
Fully integrated S/R solid 
(elform=2) 
Fully integrated S/R solid 
(elform=-2) 
Fully integrated S/R solid 
(elform=-1) 
1 point tetrahedron 
(elform=10) 
1 point nodal pressure 
tetrahedron (elform=13) 
1 point ALE 
(elform=5) 
10.928 
8.125 
3.523 
1.40 
10.976 
8.395 
3.671 
5.20 
10.972 
8.404 
3.663 
19.40 
10.976 
8.418 
3.700 
6.40 
11.088 
7.537 
2.944 
3.00 
11.017 
8.533 
3.924 
10.50 
10.892 
7.856 
2.272
The  above  displacement  and  effective  plastic  strains  results  were  obtained  from  the 
d3plot contour plots at 80.0 ms which were generated by the *DATABASE_BINARY_ 
D3PLOT keyword. 
Normalized CPU times shown in the above Penalty Method results table were normalized 
using the minimum value (the smallest value for all simulations - other contact type CPU 
times are to follow). 
Large effective plastic strains develop at the impact end of the rod due to the severe local 
mesh distortion, also resulting in reduced accuracy. 
For  these  simulations,  a  wide  range  of  CPU  times  were  associated  with  the  different 
element formulations.  The CPU time is controlled by the number of element operations 
required  for  that  particular  formulation,  the  complexity  of  the  contact-impact  approach 
and the element stable time step. 
The  one-point  quadrature  (low  order)  constant  stress  solid  (elform=1)  element 
formulation (the LS-DYNA default), the higher order, fully integrated selectively reduced 
solid (elform=2), and the higher order, fully integrated S/R solid (both so-called efficient 
and accurate formulation choices) intended to address poor aspect ratios (elform=-1 and -
2, respectively), provide roughly the same dimensional changes and maximum effective 
plastic strain. 
The  one-point  quadrature  (low  order)  tetrahedron  (elform=10)  element  formulation 
provides comparatively stiffer dimensional changes and maximum effective plastic strain 
than the constant stress solid and fully integrated element formulations.  This is probably 
due to this element formulation being prone to volumetric locking (overly stiff behavior) 
in incompressible regimes, e.g., as in plasticity. 
The  one-point  quadrature  (low  order)  nodal  pressure  tetrahedron  (elform=13)  element 
formulation  provides  a  less  stiff,  dimensional  changes  and  maximum  effective  plastic 
strain  comparison  to  that  of  the  constant  stress  solid  and  fully  integrated  element 
formulations.    This  element  formulation  has  no  volumetric  locking  under  plastic 
incompressible conditions. 
The  one  point  ALE  (elform=5)  element  formulation  provides  similar  dimensional 
changes to other element formulations.  With its nodal smoothing capability  controlling 
the  aspect  ratio  of  the  elements,  mesh  distortion  is  reduced,  yet  a  smaller  maximum 
effective  plastic  strain  (
)  is  achieved  compared  to  the  Lagrangian  elements 
ε ≅p
(
).    An  explanation  for  these  results  is  the  moderate  deformation 
to
limitation for the one point ALE formulation. 
2.272
ε =p
2.9
3.9
The LS-DYNA results for deformed shapes at 80.0 ms using penalty method contact with
Figure 27.3a – Quarter-symmetry deformed shape (penalty method) 
with effective plastic strain contouring at 80 ms (elform=1). 
Figure 27.3b – Quarter-symmetry deformed shape (penalty method)
Figure 27.3c – Quarter-symmetry deformed shape (penalty method) 
with effective plastic strain contouring at 80 ms (elform=-2). 
Figure 27.3d – Quarter-symmetry deformed shape (penalty method)
Figure 27.3e – Quarter-symmetry deformed shape (penalty method) 
with effective plastic strain contouring at 80 ms (elform=10). 
Figure 27.3f – Quarter-symmetry deformed shape (penalty method)
Figure 27.3g – Quarter-symmetry deformed shape (penalty method) 
with effective plastic strain contouring at 80 ms (elform=5). 
The  half-symmetry  deformed  shape  (penalty  method  contact),  which  illustrates  the 
different  element  deformation  for  elform=1  and  elform=5  at  80  ms,  is  given  in  Figure 
27.4. 
Figure 27.4 – Half-symmetry deformed shape (penalty method) 
for elform=1 and elform=5 at 80 ms. 
The histories of the kinetic energy, internal energy, hourglass energy, sliding energy, and 
the total energy for (elform=1) of penalty method impact are given in Figure 27.5, while 
the  histories  of  the  stable  time  step  increment  for  all  elforms  (1,2,-2,-1,10,13,5)
Figure 27.5 – Histories of the kinetic energy, internal energy, hourglass energy, 
sliding energy, and the total energy for (elform=1) of penalty method impact. 
Figure 27.6 – Histories of the stable time step increment for all elforms
Planar Rigid Boundary 
Shortening 
(mm) 
Widening 
(mm) 
Max. plastic 
strain (εp ) 
Normalized 
CPU Time 
Constant stress solid 
(elform=1) 
Fully integrated S/R solid 
(elform=2) 
Fully integrated S/R solid 
(elform=-2) 
Fully integrated S/R solid 
(elform=-1) 
1 point tetrahedron 
(elform=10) 
1 point nodal pressure 
tetrahedron (elform=13) 
1 point ALE 
(elform=5) 
10.897 
7.889 
3.243 
1.00 
10.936 
8.139 
3.366 
3.40 
10.933 
8.182 
3.394 
14.00 
10.936 
8.183 
3.405 
4.10 
11.044 
7.201 
3.057 
2.70 
10.987 
8.214 
4.288 
9.00 
10.886 
7.716 
2.272 
3.60 
The  above  displacement  and  effective  plastic  strains  results  were  obtained  from  the 
d3plot contour plots at 80.0 ms which were generated by the *DATABASE_BINARY_ 
D3PLOT keyword. 
The  more  efficient  rigid  boundary  contact  procedure  requires  less  CPU  time  (20%  to 
60%) than the penalty method for contact-impact.  The exception is the one point ALE 
multi-material formulation, where the CPU times were about the same, probably due to 
the smoothing operations control. 
For all the element formulations (except the 1 point ALE) used, the contact-impact results 
provided using the penalty method and the planar rigid boundary differ due to the contact 
methods. 
Comments  provided for  the penalty  method results  regarding element formulation  CPU 
times, the (elform=1,2,-2,-1) similarities for dimensional changes and maximum effective 
plastic strain, the (elform=10) stiffer comparison, the (elform=13) less stiff comparison, 
and the (elform=5) similarity and  difference  are  also appropriate for the  rigid  boundary 
contact results. 
The LS-DYNA results for deformed shapes at 80.0 ms using rigid boundary contact with
Figure 25.7a – Quarter-symmetry deformed shape (rigid boundary) 
with effective plastic strain contouring at 80 ms (elform=1). 
Figure 27.7b – Quarter-symmetry deformed shape (rigid boundary)
Figure 27.7c – Quarter-symmetry deformed shape (rigid boundary) 
with effective plastic strain contouring at 80 ms (elform=-2). 
Figure 27.7d – Quarter-symmetry deformed shape (rigid boundary)
Figure 27.7e – Quarter-symmetry deformed shape (rigid boundary) 
with effective plastic strain contouring at 80 ms (elform=10). 
Figure 27.7f – Quarter-symmetry deformed shape (rigid boundary)
Figure 27.7g – Quarter-symmetry deformed shape (rigid boundary) 
with effective plastic strain contouring at 80 ms (elform=5). 
The half-symmetry deformed shape (planar rigid boundary contact), which illustrates the 
different  element  deformation  for  elform=1  and  elform=5  at  80  ms,  is  given  in  Figure 
27.8. 
Figure 27.8 – Half-symmetry deformed shape (rigid boundary) 
for elform=1 and elform=5 at 80 ms. 
The histories of the kinetic energy, internal energy, hourglass energy, sliding energy, and 
the total energy for (elform=1) of rigid boundary impact are given in Figure 27.9, while 
the  histories  of  the  stable  time  step  increment  for  all  elforms  (1,2,-2,-1,10,13,5)
Figure 27.9 – Histories of the kinetic energy, internal energy, hourglass energy, 
stonewall energy, and the total energy for (elform=1) of rigid boundary impact. 
Figure 27.10 – Histories of the stable time step increment for all elforms
*TITLE 
Copper Bar Impacting a Rigidwall 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
 8.000e-02         0       0.0       0.0       0.0 
*CONTROL_TIMESTEP 
$#  dtinit    tssfac      isdo    tslimt     dt2ms      lctm     erode     ms1st 
       0.0  0.800000         0       0.0       0.0 
$#  dt2msf   dt2mslc     imscl 
       0.0         0         0 
*CONTROL_CONTACT 
$#  slsfac    rwpnal    islchk    shlthk    penopt    thkchg     orien    enmass 
  0.100000       0.0         2         0         0         0         1 
$#  usrstr    usrfrc     nsbcs    interm     xpene     ssthk      ecdt   tiedprj 
         0         0         0         0   4.00000 
$#   sfric     dfric       edc       vfc        th     th_sf    pen_sf 
       0.0       0.0       0.0       0.0       0.0       0.0       0.0 
$#  ignore    frceng   skiprwg 
         0         0         0 
*CONTROL_ENERGY 
$#    hgen      rwen    slnten     rylen 
         2         2         2         2 
*DATABASE_GLSTAT 
$#      dt    binary 
5.0000e-04         1 
*DATABASE_MATSUM 
$#      dt    binary 
5.0000e-04         1 
*DATABASE_SLEOUT 
$#      dt    binary 
5.0000e-04         1 
*DATABASE_RWFORC 
$#      dt    binary 
5.0000e-04         1 
*DATABASE_BINARY_D3PLOT 
$# dt/cycl   lcdt/nr      beam     npltc    psetid 
1.0000e-03 
*PART 
$# title                                                                         
material type # 3 (Kinematic/Isotropic Elastic-Plastic)                          
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         1         1         1         0         1 
*SECTION_SOLID 
$#   secid    elform       aet 
         1         1 
*MAT_PLASTIC_KINEMATIC 
$#     mid        ro         e        pr      sigy      etan      beta 
         1 8.930e-03 1.170e+05   0.35000 4.000e+02 1.000e+02       0.0 
$#     src       srp        fs        vp 
       0.0       0.0       0.0       0.0 
*HOURGLASS 
$#    hgid       ihq        qm       ibq        q1        q2        qb        qw 
         1         0       0.0         0       0.0       0.0       0.0       0.0 
*PART 
$# title                                                                         
material type # 20 (Rigid)                                                       
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         2         2         2         0         2 
*SECTION_SHELL 
$#   secid    elform      shrf       nip     propt   qr/irid     icomp     setyp 
         2         2       0.0         0         0       0.0 
$#      t1        t2        t3        t4      nloc     marea 
  0.100000  0.100000  0.100000  0.100000         0       0.0 
*MAT_RIGID 
$#     mid        ro         e        pr         n    couple         m 
         2 8.930e-03 1.170e+05   0.35000       0.0       0.0       0.0
1.000000         7         7 
$#lco or a1       a2        a3        v1        v2        v3 
       0.0       0.0       0.0       0.0       0.0       0.0 
*HOURGLASS 
$#    hgid       ihq        qm       ibq        q1        q2        qb        qw 
         2         0       0.0         0       0.0       0.0       0.0       0.0 
*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_TITLE 
$#     cid                                                                 title 
         1copper bar-rigidwall interface                                         
$#    ssid      msid     sstyp     mstyp    sboxid    mboxid       spr       mpr 
         1         2         3         3 
$#      fs        fd        dc        vc       vdc    penchk        bt        dt 
       0.0       0.0       0.0       0.0       0.0         0       0.0       0.0 
$#     sfs       sfm       sst       mst      sfst      sfmt       fsf       vsf 
       0.0       0.0       0.0       0.0       0.0       0.0       0.0       0.0 
$#    soft    sofscl    lcidab    maxpar     sbopt     depth     bsort    frcfrq 
         2  0.100000         0     1.025       0.0         2        10         1 
$#  penmax    thkopt    shlthk     snlog      isym     i2d3d    sldthk    sldstf 
       0.0         0         1         0         0         0       0.0       0.0 
$#    igap    ignore 
         2         0 
*INITIAL_VELOCITY_GENERATION 
$#      id      styp     omega        vx        vy        vz     ivatn      icid 
         1         2       0.0       0.0       0.0   -227.00         0         0 
$#      xc        yc        zc        nx        ny        nz     phase    irigid 
       0.0       0.0       0.0       0.0       0.0       0.0         0         0 
*ELEMENT_SOLID 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
       1       1       1      10      11       2     306     315     316     307 
   10368       1   10900   10683   10684   10748   11205   10988   10989   11053 
*ELEMENT_SHELL 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
   10369       2   11299   11300   11287   11286       0       0       0       0 
   10512       2   11453   11454   11441   11440       0       0       0       0 
*NODE 
$#   nid               x               y               z      tc      rc 
       1        1.131371        1.131371           0.000       0       0 
   11285       -0.848528       -0.848528       32.400000       0       0 
   11286       10.000000      -10.000000       -0.100000       0       0 
   11454      -10.000000       10.000000       -0.100000       0       0 
*END 
Notes: 
1.  If  a  part  is  comprised  entirely  of  tetrahedrons,  there  are  several  tetrahedral 
formulations  to  choose  from,  each  with  various  pros  and  cons.    Any  of  these 
formulations are preferable to using degenerate, elform=1 tetrahedrons.  Two popular 
choices  are  (a)  elform=10  which  is  1  point  tetrahedron  with  4  nodes,  but  prone  to 
volumetric locking (overly stiff behavior) in incompressible regimes, e.g., as in metal 
plasticity, and (b) elform=13 which is a 1 point nodal pressure tetrahedron developed 
for bulk metal forming; elform=13 is identical with elform=10 with addition of nodal 
pressure  averaging  that  significantly  decreases  volumetric  locking.    There  are  also 
two  relatively  new  10-noded  tetrahedron,  elform=16  and  17  which  have  not  been 
widely used. 
2.  To  convert  from  a  Lagrangian  simulation  to  an  ALE,  the  user  needs  to  add  the
logic  (dct),  cycle  between  advection  (nadv),  advection  method  (meth),  smoothing 
weight factors (afac thru efac), etc.: 
*CONTROL_ALE 
$#     dct      nadv      meth      afac      bfac      cfac      dfac      efac 
        -1         1         2  0.500000  0.500000       0.0       0.0       0.0 
$#   start       end     aafac     vfact    vlimit       ebc      pref 
       0.0 1.000e+20  1.000000 1.000e-06       0.0         0       0.0 
and modify the element formulation choice: 
*SECTION_SOLID 
$#   secid    elform       aet 
         1         5 
3.  Hexahedral elements with reasonable aspect ratios should be used for the initial ALE 
mesh.  Degenerate element shapes, such as tetrahedrons and pentahedrons, should be 
avoided as they lead to reduced accuracy and perhaps numerical instability during the 
advection. 
4.  The  viscous  contact  damping  parameter,  vdc,  on  card  2  of  the  *CONTACT_ 
AUTOMATIC_SURFACE_TO_SURFACE  keyword  is  zero  by  default.    Contact 
damping is often beneficial in reducing high-frequency oscillation of contact forces in 
crash or impact simulations.  In contacts involving soft materials such as foams and 
honeycombs,  instabilities  exist  due  to  contact  oscillations.    Using  a  value  of  vdc 
between  40-60  (corresponding  to  40%  to  60%  of  critical  damping),  improves 
stability;  however,  it  may  be  necessary  to  reduce  the  time  step  scale  factor.  
Generally,  a  smaller  value  of  vdc,  say  equal  to  20,  is  recommended  when  metals, 
which have similar material stiffnesses, interact. 
5.  Contact-impact results using penalty method and planar rigid boundaries can possible 
differ  due  to  their  approaches.    The  penalty  method  consists  of  placing  normal 
interface  springs  between  all  penetrating  nodes  and  the  contact  surface.    The  rigid 
boundary  contact  procedure  for  stopping  nodes  uses  a  constraint  method  which 
represents  a  perfectly  plastic  impact  that  results  in  an  irreversible  energy  loss.    The 
total  energy  dissipated  is  found  by  taking  the  difference  between  the  total  kinetic 
energy of all the nodal points slaved to the rigid wall before and after the impact with 
the wall.  The advantage of the constraint method is that it guarantees the node to lie 
on the positive side of the rigidwall (no penetration). 
6.  To move from the contact-impact model used by the penalty method, i.e. that with a 
meshed  rigid  wall,  to  a  planar  rigid  boundary  model,  the  user  needs  to  remove  the 
following entries used to represent the contact-impact and the meshed rigid wall: 
*CONTROL_CONTACT 
$#  slsfac    rwpnal    islchk    shlthk    penopt    thkchg     orien    enmass 
  0.100000       0.0         2         0         0         0         1 
$#  usrstr    usrfrc     nsbcs    interm     xpene     ssthk      ecdt   tiedprj 
         0         0         0         0   4.00000 
$#   sfric     dfric       edc       vfc        th     th_sf    pen_sf 
       0.0       0.0       0.0       0.0       0.0       0.0       0.0
$# title                                                                         
material type # 20 (Rigid)                                                       
$#     pid     secid       mid     eosid      hgid      grav    adpopt      tmid 
         2         2         2         0         2 
*SECTION_SHELL 
$#   secid    elform      shrf       nip     propt   qr/irid     icomp     setyp 
         2         2       0.0         0         0       0.0 
$#      t1        t2        t3        t4      nloc     marea 
  0.100000  0.100000  0.100000  0.100000         0       0.0 
*MAT_RIGID 
$#     mid        ro         e        pr         n    couple         m 
         2 8.930e-03 1.170e+05   0.35000       0.0       0.0       0.0  
$#     cmo      con1      con2       
  1.000000         7         7 
$#lco or a1       a2        a3        v1        v2        v3         
       0.0       0.0       0.0       0.0       0.0       0.0 
*HOURGLASS 
$#    hgid       ihq        qm       ibq        q1        q2        qb        qw 
         2         0       0.0         0       0.0       0.0       0.0       0.0 
*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_TITLE 
$#     cid                                                                 title 
         1copper bar-rigidwall interface                                
$#    ssid      msid     sstyp     mstyp    sboxid    mboxid       spr       mpr 
         1         2         3         3 
$#      fs        fd        dc        vc       vdc    penchk        bt        dt 
       0.0       0.0       0.0       0.0      20.0         0       0.0       0.0 
$#     sfs       sfm       sst       mst      sfst      sfmt       fsf       vsf 
       0.0       0.0       0.0       0.0       0.0       0.0       0.0       0.0 
$#    soft    sofscl    lcidab    maxpar     sbopt     depth     bsort    frcfrq 
         2  0.100000         0     1.025       0.0         2        10         1 
$#  penmax    thkopt    shlthk     snlog      isym     i2d3d    sldthk    sldstf 
       0.0         0         1         0         0         0       0.0       0.0 
$#    igap    ignore 
         2         0 
*ELEMENT_SHELL 
$#   eid     pid      n1      n2      n3      n4      n5      n6      n7      n8 
   10369       2   11299   11300   11287   11286       0       0       0       0 
   10512       2   11453   11454   11441   11440       0       0       0       0 
*NODE 
$#   nid               x               y               z      tc      rc 
   11286       10.000000      -10.000000       -0.100000       0       0 
   11454      -10.000000       10.000000       -0.100000       0       0 
and  replace  them  with  the  following  planar  rigid  boundary  entry  (the  user  can  also 
include the rigid wall force entry if desired): 
*DATABASE_RWFORC 
$#      dt    binary 
5.0000e-04         1 
*RIGIDWALL_PLANAR 
$#    nsid    nsidex     boxid    offset     birth     death     rwksf 
         0         0         0 
$#      xt        yt        zt        xh        yh        zh      fric      wvel
Implicit Studies: 
NIKE3D  (implicit  dynamics  solver)  was  used  by  Ferencz  [1989]  with  the  computation 
divided into 80 time steps of 1 microsecond and nodal boundary conditions constraining 
the impacting face to lie on the global X-Y plane.  The half-symmetry deformed shape, at 
80 ms (final state), is shown in Figure 27.11. 
NIKE3D uses an element formulation, similar to the selected reduced integration of LS-
DYNA (elform=2), defined as B-Bar method.  The selective reduced integration splits the 
stress tensor into deviatoric and dilatation (mean) parts, whereas the B-Bar method splits 
the B matrix (a strain modification) into dilatational and deviatoric parts. 
The  contact  of  the  deformable  body  and  the  rigid  wall  can  be  modeled  in  one  of  the 
following ways in this study: 
•  using nodal boundary conditions which constrain the impacting face to remain on the 
• 
rigid wall, 
rigid  wall  (*RIGIDWALL_PLANAR),  which  provides  an  easy  way  to  treat  contact 
between a rigid-flat surface and the nodes of a deformable body. 
In general, there are two different methods that are available in LS-DYNA to treat nodes 
impacting a  rigid wall.  The first method, which  is the default method, is the constraint 
type that is used for all deformable nodes impacting a rigid wall.  The second (optional) 
method  is  the  penalty  approach  that  is  used  for  all  rigid  nodes  or  optional  deformable 
nodes impacting  the  rigid wall.  The  primary difference  between  the  two methods  is  in 
the conservation of energy and momentum.  If using the implicit solver, only the penalty 
approach method is available. 
The default constraint method does not conserve momentum and the energy.  This is due 
to the fact that when a deformable node is found to penetrate a rigidwall, its velocity is 
immediately  reset  to  zero  and  is  moved  back  onto  the  surface  of  the  rigidwall.    The 
advantage  of  the  constraint  method  is  that  it  always  guarantees  the  node  to  lie  on  the 
positive side of the rigidwall (no penetration). 
The penalty method (optional for explicit solver/default for implicit solver) for rigid walls 
uses a scale factor that can be adjusted (default is 1.0) by modifying the rwskf parameter 
on  *RIGIDWALL_PLANAR  keyword.    This  works  the  same  as  the  contact-impact 
interface treatment.  When a deformable or a rigid node is found to penetrate a rigidwall, 
the penetrated distance normal to the rigid wall is computed and is resisted by applying a 
force that is proportional to the computed distance multiplied by a stiffness factor that is 
based on the material of the impacting node and the dimensions of the attached element.
Figure 27.11 – Half-symmetry deformed shape (Ferencz [1989]) at 80 ms (final state). 
Analysis Summary: 
Dim. 
Type 
Load  Material  Geometry  Contact 
Solver 
3D  Dynamic  Velocity 
Non-
linear 
Non-
linear 
SPC's 
Implicit 
and 
Dim. 
Type 
Load  Material  Geometry  Contact 
Solver 
Solution 
Method 
 2-Nonlinear 
w/BFGS 
Solution 
Method 
3D  Dynamic  Velocity 
Non-
linear 
Non-
linear 
R.Wall 
(penalty) 
Explicit/ 
Implicit 
 2-Nonlinear 
w/BFGS 
Element Type:
Different Considerations from Explicit Solver: 
The  contact  of  the  deformable  body  and  the  rigid  wall  can  be  modeled  in  one  of  the 
following ways in this study: 
•  using nodal boundary conditions which constrain the impacting face to remain on the 
• 
rigid wall, 
rigid  wall  (*RIGIDWALL_PLANAR),  which  provides  an  easy  way  to  treat  contact 
between a rigid-flat surface and the nodes of a deformable body. 
Studies 1 and 2: 
•   NIKE3D and LS-DYNA (each using implicit dynamics solver) Comparison, and 
•   Implicit LS-DYNA Convergence, 
with nodal boundary conditions constraining the impacting face for both studies. 
Nodal Boundary (SPC's) 
Shortening 
(mm) 
Widening 
(mm) 
Max. plastic 
strain (εp ) 
Normalized 
CPU Time 
B-Bar solid (NIKE3D) - 
80 time steps 
Fully integrated S/R solid 
80 time steps 
Fully integrated S/R solid 
160 time steps 
Fully integrated S/R solid 
320 time steps 
Fully integrated S/R solid 
400 time steps 
Fully integrated S/R solid 
480 time steps 
Fully integrated S/R solid 
640 time steps 
Fully integrated S/R solid 
800 time steps 
11.446 
7.68 est. 
2.248 
- 
11.313 
6.111 
2.432 
3.35 
11.150 
7.468 
3.126 
6.54 
11.029 
7.730 
3.080 
13.10 
11.005 
7.765 
3.084 
16.84 
10.989 
7.784 
3.084 
19.50 
10.974 
7.798 
3.090 
25.90 
10.967 
7.805 
3.092
The above displacement and effective plastic strain results were obtained from the d3plot 
contour  plots  at  80.0  ms  which  were  generated  by  the  *DATABASE_BINARY_ 
D3PLOT keyword. 
Normalized  CPU  times  shown  in  the  above  Nodal  Boundary  Condition  (SPC's)  results 
table were normalized using the explicit fully integrated S/R solid (elform=2) value. 
In the implicit solver direct comparison (80 time steps) of NIKE3D which uses the B-Bar 
element  formulation  and  the  selected  reduced  integration  element  formulation  of  LS-
DYNA  (elform=2),  similar  maximum  effective  plastic  strain  results  (
  vs. 
ε =p
) and length shortening (11.446 mm vs. 11.313 mm) are obtained.  For some 
unexplained reason, the widening profiles (7.680 mm vs. 6.111 mm) differ significantly. 
2.248
2.432
ε =p
2.432
) is significantly less than the explicit solver value (
The  maximum  effective  plastic  strain  obtained  using  the  LS-DYNA  implicit  solver 
ε =p
(
 - initial work 
with  penalty  contact  condition).    This  is  believed  to  be  due  to  the  relatively  large  time 
step  increment  used  (only  80  steps)  which  fails  to  capture  the  correct  dynamics  of  the 
simulation.  It is shown in above table that increasing the number of time steps (reducing 
the time step increment) allows the implicit solver to more accurately capture the rate of 
material  deformation  (plastic  flow)  and  appears  to  be  converging  to  a  unique  solution 
ε =p
(
 and 7.810 mm) with a consistent shape profile. 
3.366
3.100
ε =p
The  half-symmetry  deformed  shape  (nodal  boundary  constraint)  with  widening  profiles 
and effective plastic strain contouring for selected implicit integration time step sizes at 
80 ms, are given in Figures 27.12 (80 time steps), 27.13 (160 time steps), and 27.14 (640 
time  steps).    Figure  27.12  provides  a  LS-DYNA  deformed  shape  (80  time  steps) 
comparison  with  the  NIKE3D  result  (80  time  steps)  shown  in  Figure  27.11.    Together, 
 and 7.468 mm), and 27.14 
Figures 27.12 (
ε =p
(
 and 7.798 mm) illustrate the  LS-DYNA  converging results  with increasing 
the number of time steps (reducing the time step increment). 
 and 6.111 mm), 27.13 (
3.090
3.126
2.432
ε =p
ε =p
Unfortunately, as is shown in above table, the CPU time becomes a deterrent when using 
implicit  dynamics  solvers.    Thus,  the  explicit  solver  is  often  favored  for  these  types  of 
high  deformation,  impact  simulations  due  to  its  ability  to  provide  efficient  and  stable
Figure 27.12 – Half-symmetry widening and effective plastic strain contouring with 
nodal boundary conditions - 80 time steps. 
Figure 27.13 – Half-symmetry widening and effective plastic strain contouring with
Figure 27.14 – Half-symmetry widening and effective plastic strain contouring with 
nodal boundary conditions - 640 time steps. 
Input deck: 
*KEYWORD 
*TITLE 
Copper Bar Impacting a Rigidwall 
*CONTROL_IMPLICIT_DYNAMICS 
$#   imass     gamma      beta 
         1  0.500000  0.250000 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form 
         1   0.00100         0         0         0 
$         1   0.00050         0         0         0 
$         1   0.00025         0         0         0 
$         1   0.00020         0         0         0 
$         1 0.0001666         0         0         0 
$         1 0.0001250         0         0         0 
$         1   0.00010         0         0         0 
*CONTROL_IMPLICIT_SOLVER 
$#  lsolvr   prntflg    negeig     order      drcm    drcprm    autospc    aspctl 
         4         2         2         0         1         0          1         0 
$#  lcpack 
         2 
*CONTROL_IMPLICIT_SOLUTION 
$#  nsolvr    ilimit    maxref     dctol     ectol     rctol       stol    abstol 
         2        11        15    0.0010    0.0100  1.00e+10   0.900000  1.00e-10 
$#   dnorm    diverg     istif   nlprint    nlnorm   d3itctl      cpchk 
         2         1         1         2 
$#  arcctl    arcdir    arclen     rcmth    arcdmp 
         0         1       0.0         1         2 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas
3         0         3       0.0       0.0       0.0 
*END 
Notes: 
Studies 3 and 4: 
•   LS-DYNA  Explicit  Solver  (with  rigid  wall  constraint  method  contact)  and  Implicit 
Dynamics Solver (with rigid wall penalty method contact) Comparison, and 
•   Implicit LS-DYNA Convergence. 
Planar Rigid Boundary 
Shortening 
(mm) 
Widening 
(mm) 
Max. plastic 
strain (εp ) 
Normalized 
CPU Time 
Fully integrated S/R solid 
Explicit - 9883 time steps 
Fully integrated S/R solid 
Implicit - 80 time steps 
Fully integrated S/R solid 
Implicit - 160 time steps 
Fully integrated S/R solid 
Implicit - 320 time steps 
Fully integrated S/R solid 
Implicit - 400 time steps 
Fully integrated S/R solid 
Implicit - 480 time steps 
Fully integrated S/R solid 
Implicit - 640 time steps 
Fully integrated S/R solid 
Implicit - 800 time steps 
Fully integrated S/R solid 
Implicit - 1600 time steps 
Fully integrated S/R solid 
Implicit - 3200 time steps 
10.936 
8.139 
3.366 
1.00 
11.155 
7.083 
2.821 
3.35 
11.285 
7.326 
3.109 
6.54 
11.216 
7.502 
3.235 
13.10 
11.179 
7.534 
3.270 
16.84 
11.166 
7.550 
3.274 
19.50 
11.045 
8.503 
3.586 
25.90 
11.033 
8.517 
3.644 
33.38 
11.023 
8.542 
3.680 
67.30 
11.022 
8.545 
3.696
The above displacement and effective plastic strain results were obtained from the d3plot 
contour  plots  at  80.0  ms  which  were  generated  by  the  *DATABASE_BINARY_ 
D3PLOT keyword. 
Normalized  CPU  times  shown  in  the  above  Rigid  Wall  Planar  results  table  were 
normalized using the explicit fully integrated S/R solid (elform=2) value. 
ε =p
2.821
As  for  the  previous  nodal  boundary  condition  method,  the  maximum  effective  plastic 
strain  (
)  and  widening  profile  (7.083  mm)  for  the  80  time  step  solution  are 
ε =p
roughly 15% less than the explicit results (
 and 8.139 mm).  As before, this is 
believed to be due to the relatively large time step increment used (only 80 steps) which 
fails  to  capture  the  correct  dynamics  of  the  simulation.    It  is  shown  that  increasing  the 
number  of  time  steps  (reducing  the  time  step  increment)  allows  the  solver  to  better 
capture  the  rate  of  material  deformation  (plastic  flow)  which  appears  to  be  converging 
ε =p
(
 and 7.550 mm) over a range of time steps studied. 
3.366
3.274
For some unexplained reason, starting with the 640 time step solution, there is a further 
increase in maximum effective plastic strain and widening results and a distinct change in 
the  widening  profile  with  the  outer  row  of  nodes  now  turning  more  upward.    The 
ε =p
  and  8.545  mm)  appear  to  be  converging,  though 
corresponding  results  (
greater than those provided by the explicit solver (
 and 8.139 mm) which also 
has the outer row of nodes turning slightly upward. 
3.366
3.696
ε =p
The  half-symmetry  deformed  shape  (planar  rigid  boundary)  with  widening  profiles  and 
effective  plastic  strain  contouring  for  selected  implicit  integration  time  step  sizes  at  80 
ms, are  given in Figures 27.15 (explicit), 27.16 (80 time steps), 27.17 (160 time steps), 
and 27.18 (640 time steps).  Figure 27.15 provides a LS-DYNA widening and effective 
  and  8.139  mm)  for  the  explicit  solver.    Together, 
plastic  strain  results  (
Figures 27.16 (
 and 7.326 mm), and 27.18 
ε =p
(
 and 8.503 mm) illustrate the  LS-DYNA  converging  results for  the  implicit 
solver with increasing the number of time steps (reducing the time step increment). 
 and 7.083 mm), 27.17 (
3.366
2.821
3.109
3.586
ε =p
ε =p
ε =p
Unfortunately, as is shown in above table, the CPU time becomes a deterrent when using 
implicit  dynamics  solvers.    Thus,  the  explicit  solver  is  often  favored  for  these  types  of 
high  deformation,  impact  simulations  due  to  its  ability  to  provide  efficient  and  stable
Figure 27.15 – Half-symmetry widening and effective plastic strain contouring with 
rigid boundary condition - explicit. 
Figure 27.16 – Half-symmetry widening and effective plastic strain contouring with
Figure 27.17 – Half-symmetry widening and effective plastic strain contouring with 
rigid boundary condition - 160 time steps. 
Figure 27.18 – Half-symmetry widening and effective plastic strain contouring with
*TITLE 
Copper Bar Impacting a Rigidwall 
*CONTROL_IMPLICIT_DYNAMICS 
$#   imass     gamma      beta 
         1  0.500000  0.250000 
*CONTROL_IMPLICIT_GENERAL 
$#  imflag       dt0    imform      nsbs       igs     cnstn      form 
         1   0.00100         0         0         0 
$         1   0.00050         0         0         0 
$         1   0.00025         0         0         0 
$         1   0.00020         0         0         0 
$         1 0.0001666         0         0         0 
$         1 0.0001250         0         0         0 
$         1   0.00010         0         0         0 
$         1   0.00005         0         0         0 
$         1  0.000025         0         0         0 
*CONTROL_IMPLICIT_SOLVER 
$#  lsolvr   prntflg    negeig     order      drcm    drcprm    autospc    aspctl 
         4         2         2         0         1         0          1         0 
$#  lcpack 
         2 
*CONTROL_IMPLICIT_SOLUTION 
$#  nsolvr    ilimit    maxref     dctol     ectol     rctol       stol    abstol 
         2        11        15    0.0010    0.0100  1.00e+10   0.900000  1.00e-10 
$#   dnorm    diverg     istif   nlprint    nlnorm   d3itctl      cpchk 
         2         1         1         2 
$#  arcctl    arcdir    arclen     rcmth    arcdmp 
         0         1       0.0         1         2 
*CONTROL_TERMINATION 
$#  endtim    endcyc     dtmin    endeng    endmas 
 8.000e-02         0       0.0       0.0       0.0 
*RIGIDWALL_PLANAR 
$#    nsid    nsidex     boxid    offset     birth     death     rwksf 
         0         0         0                                     5.0 
*END

Table of Contents 
page 
1. 
Introduction............................................................................................................................... 1-1 
2.  Units........................................................................................................................................... 2-1 
3.  Getting Started........................................................................................................................... 3-1 
3.1 
3.2 
3.3 
Problem Definition........................................................................................................... 3-1 
Input File Preparation..................................................................................................... 3-1 
LS-DYNA solution ........................................................................................................... 3-4 
4.  The Next Step ............................................................................................................................ 4-1 
4.1 
4.2 
Explicit Analysis (problem ex01.k)................................................................................. 4-1 
Implicit Analysis (problem im01.k)................................................................................ 4-3 
4.3  Heat Transfer Analysis (problem th01.k)...................................................................... 4-5
List of Examples 
Example 4-1 Aluminum cube deformation, explicit method (file: ex01.k) 
Example 4-2 Aluminum cube deformation, implicit method (file: im01.k) 
Example 4-3 Aluminum cube transient heat transfer analysis (file: th01.k) 
Example 4-4 Aluminum cube coupled thermal-stress solution (file: cp01.k) 
page 
4-2 
4-3
LS-DYNA 
Introduction 
1.  Introduction 
LS-DYNA is used to solve multi-physics problems including solid mechanics, heat transfer, and 
fluid dynamics either as separate phenomena or as coupled physics, e.g., thermal stress or fluid 
structure interaction. This manual presents  “very simple” examples to be used as templates (or 
recipes). 
This manual should be used side-by-side with the “LS-DYNA Keyword User’s Manual”. The 
keyword input provides a flexible and logically organized database. Similar functions are grouped 
together under the same keyword. For example, under the keyword, *ELEMENT, are included solid, 
beam, and shell elements. The keywords can be entered in an arbitrary order in the input file. 
However, for clarity in this manual, we will conform to the following general block structure and 
enter the appropriate keywords in each block. 
1.  define solution control and output parameters 
2.  define model geometry and material parameters
LS-DYNA 
Units 
2.  Units 
LS-DYNA requires a consistent set of units to be used. All parameters in this manual are in SI units. 
length   
General 
• 
•  mass 
temperature 
• 
time 
• 
•  pressure 
Mechanical units 
•  density  
•  Modulus of elasticity   
•  yield stress 
•  coefficient of expansion 
Thermal units 
•  heat capacity   
• 
•  heat generation rate 
thermal conductivity   
[m] 
[kg] 
[K] 
[sec] 
[Pa] 
[kg/m3] 
[Pa] 
[Pa] 
[m/m K] 
[J/kg K] 
[W/m K]
LS-DYNA 
Getting Started 
3.  Getting Started 
3.1  Problem Definition 
Consider the deformation of an aluminum block sitting on the floor with a pressure applied to the top 
surface. 
P = 70.e+05 Pa 
Aluminum 1100-O 
density  
modulus of elasticity   
Poisson Ratio   
coefficient of expansion 
heat capacity 
thermal conductivity   
2700 kg/m3 
70.e+09 Pa 
0.3 
23.6e-06 m/m K 
900 J/kg K 
220 W/m K 
1m
3.2  Input File Preparation 
The first step is to create a mesh and define node points. Since we are just getting started, we will 
define the mesh as consisting of only 1 element and 8 node points as shown in the following figure. 
Also, we will use default values for many of the parameters in the input file, and therefore not have 
to enter them. 
5 
1 
6 
2 
8 
4 
7 
3 
The “LS-DYNA Keyword User’s 
Manual” should be read side-by-side 
with this manual. 
The following steps are required to create the finite element model input file. 
*KEYWORD 
The first line of the input file must begin with *KEYWORD. This identifies the file as 
containing the “keyword” format instead of the “structured” format which can also 
be used . 
The first input block is used to define solution control and output parameters. As a minimum, the
LS-DYNA 
Getting Started 
will apply the pressure load as a ramp from 0 Pa to 70.e+05 Pa during a time interval of 1 second. 
Therefore, the termination time is 1 second. Additionally, one of the many output options should be 
used to control the printing interval of results (e.g., *DATABASE_BINARY_D3PLOT). We will 
print the results every 0.1 seconds. 
*CONTROL_TERMINATION 
        1. 
*DATABASE_BINARY_D3PLOT 
        .1 
The second input block is used to define the model geometry, mesh, and material parameters. The 
following description and map may help to understand the data structure in this block. We have 1 
part, the aluminum block, and use the *PART keyword to begin the definition of the finite element 
model. The keyword *PART contains data that points to other attributes of this part, e.g., material 
properties. Keywords for these other attributes, in turn, point elsewhere to additional attribute 
definitions. The organization of the keyword input looks like this.  
*PART 
pid  sid  mid 
*SECTION_SOLID  
sid 
*MAT_ELASTIC 
mid  ρ 
E 
µ 
*ELEMENT_SOLID  
eid  pid  nid 
*NODE 
nid  x 
y 
z 
The LS-DYNA Keyword User Manual should be consulted at this time for a description of the 
keywords used above. A brief description follows: 
*PART 
We have 1 part identified by part identification (pid=1). This part has 
attributes identified by section identification (sid=1) and material 
identification (mid=1). 
*SECTION_SOLID  Parts identified by (sid=1) are defined as constant stress 8 node brick 
elements by this keyword. 
*MAT_ELASTIC 
Parts identified by (mid=1) are defined as an elastic material with a density
LS-DYNA 
Getting Started 
*ELEMENT_SOLID  Eight node solid brick elements identified by element identification (eid=1) 
have the attributes of (pid=1) and are defined by the node list (nid) 
*NODE 
The node identified by (nid) has coordinates x,y,z. 
Our finite element model consists of 1 element, 8 nodes, and 1 material. Keeping the above in mind, 
the data entry for this block looks like this. 
*PART 
aluminum block 
         1         1         1 
*SECTION_SOLID 
         1 
*MAT_ELASTIC 
         1     2700.   70.e+09        .3 
*ELEMENT_SOLID 
       1       1       1       2       3       4       5       6       7       8
*NODE 
       1              0.              0.              0.       7       7 
       2              1.              0.              0.       5       0 
       3              1.              1.              0.       3       0 
       4              0.              1.              0.       6       0 
       5              0.              0.              1.       4       0 
       6              1.              0.              1.       2       0 
       7              1.              1.              1.       0       0 
       8              0.              1.              1.       1       0 
The third input block is used to define boundary conditions and time dependent load curves. We are 
applying a load of 70.e+05 Pa to the top surface of the block defined by nodes 5-6-7-8. We will 
ramp the load up from 0 Pa to 70.e+05 Pa during a time interval of 1 second. 
Note that the first data entry in *LOAD_SEGMENT is a load curve 
identification number (lcid=1) which points to the load curve defined by 
the keyword *DEFINE_CURVE having that same (lcid) identification 
number.  
*LOAD_SEGMENT 
         1        1.        0.         5         6         7         8 
*DEFINE_CURVE 
*END  
         1 
                  0.                  0. 
                  1.             70.e+05 
The last line in the input file must have the keyword *END. 
*END
LS-DYNA 
Getting Started 
3.3  LS-DYNA solution 
The vertical and horizontal displacement of node 7, calculated by LS-DYNA, are shown in the 
following 2 graphs. The solution to this simple problem can be calculated analytically. The LS-
DYNA solution compares exactly with the analytical solution.  
The vertical displacement 
due to a 70.0e+05 Pa 
pressure load can be 
calculated by 
=∆
Pl
=
(
)( )
70
105
+
(
)
70
09
+
=
1.0e-04 m 
The horizontal displacement 
is 
lh µ
=∆=∆
(
)(
.03.0
0001
) =
LS-DYNA 
The Next Step 
4.  The Next Step 
This chapter builds on the simple example presented in the previous chapter. First, more detail is 
given about solving this problem using explicit analysis in section 4.1. Explicit analysis is well 
suited to dynamic simulations such as impact and crash analysis, but it can become prohibitively 
expensive to conduct long duration or static analyses. Static problems, such as sheet metal spring 
back after forming, are one application area for implicit analysis. Implicit analysis is presented in 
section 4.2. The difference between explicit and implicit is described. The problem is then presented 
as a heat transfer problem in section 4.3 and finally as a coupled thermal-stress problem in section 
4.4. 
4.1  Explicit Analysis (problem ex01.k) 
Explicit refers to the numerical method used to represent and solve the time derivatives in the 
momentum and energy equations. The following figure presents a graphical description of  
 time t+∆t .    .    .
.    .    .
 time t
 n1    n2     n3
explicit time integration. The displacement of node n2 at time level t+∆t is equal to known values of 
the displacement at nodes n1, n2, and n3 at time level t. A system of explicit algebraic equations are 
written for all the nodes in the mesh at time level t+∆t. Each equation is solved in-turn for the 
unknown node point displacements. Explicit methods are computational fast but are conditionally 
stable. The time step, ∆t, must be less than a critical value or computational errors will grow 
resulting in a bad solution. The time step must be less than the length of time it takes a signal 
traveling at the speed of sound in the material to traverse the distance between the node points. The 
critical time step for this problem can be calculated by 
∆t ≤
∆x
=
=
∆x
1.
70. ∗10
2700.
= 1.96 ∗10 −4 sec   
To be safe, the default value used by LS-DYNA is 90% of this value or 1.77e-04 sec. Therefore, this 
problem requires 5,658 explicit time steps as compared with 10 implicit time steps .  
Note that the time step and scale factor can be set using the keyword *CONTROL_TIMESTEP. 
The input file for the 1-element aluminum cube example problem, presented in Chapter 3, is
LS-DYNA 
The Next Step 
Example 4-1 Aluminum cube deformation, explicit method (file: ex01.k) 
PID 
MID
SECID 
*KEYWORD 
*TITLE 
ex01.k – explicit analysis, problem 1 
$ 
$---------------  define solution control and output parameters ---------------- 
$ 
*CONTROL_TERMINATION 
        1. 
*DATABASE_BINARY_D3PLOT 
        .1 
$ 
$---------------  define model geometry and material parameters ---------------- 
$ 
*PART 
aluminum block 
         1         1         1 
*SECTION_SOLID 
         1 
*MAT_ELASTIC 
         1     2700.   70.e+09        .3 
*NODE 
       1              0.              0.              0.       7       7 
       2              1.              0.              0.       5       0 
       3              1.              1.              0.       3       0 
       4              0.              1.              0.       6       0 
       5              0.              0.              1.       4       0 
NID 
       6              1.              0.              1.       2       0 
       7              1.              1.              1.       0       0 
       8              0.              1.              1.       1       0 
*ELEMENT_SOLID 
       1       1       1       2       3       4       5       6       7       8 
$ 
$----------------  define boundary conditions and load curves ------------------ 
$ 
*LOAD_SEGMENT 
         1        1.        0.         5         6         7         8 
*DEFINE_CURVE 
         1 
                  0.                  0. 
                  1.             70.e+05 
*END 
LCID
LS-DYNA 
The Next Step 
4.2  Implicit Analysis (problem im01.k) 
Implicit refers to the numerical method used to represent and solve the time derivatives in the 
momentum and energy equations. The following figure presents a graphical description of  
 time t+∆t .    .    .
.    .    .
 time t
 n1    n2     n3
implicit time integration. The displacement of node n2 at time level t+∆t is equal  to known values of 
the displacement at nodes n1, n2, and n3 at time level t, and also the unknown displacements of 
nodes n1 and n3 at time level t+∆t. This results in a system of simultaneous algebraic equations that 
are solved using matrix algebra (e.g., matrix inversion). The advantage of this approach is that it is 
unconditionally stable (i.e., there is no critical time step size). The disadvantage is the large 
numerically effort required to form, store, and invert the system of equations. Implicit simulations 
typically involve a relatively small number of computationally expensive time steps. 
The keyword *CONTROL_IMPLICIT_GENERAL is used to activate the implicit method. The 
second entry on this card is the time step. For this example the time step is 0.1 sec. Therefore, a total 
of 10 implicit time steps will be taken to solve this problem. The results are identical to those 
obtained by the explicit method as shown in Sec 3.3.  
For small problems, such as this 1 element example, most of the computer time is spent performing 
IO operations in reading the data and writing the output files. Very little CPU time is spent solving 
the problem. No conclusions should be made concerning the execution speed of explicit versus 
implicit methods on this problem. 
Example 4-2 Aluminum cube deformation, implicit method (file: im01.k) 
*KEYWORD 
*TITLE 
im01.k – implicit analysis – problem 1 
$ 
$-------------------------- implicit solution keywords ------------------------- 
$ 
*CONTROL_IMPLICIT_GENERAL 
This keyword turns on the implicit method
1 
.1 
$ 
$---------------  define solution control and output parameters ---------------- 
$ 
*CONTROL_TERMINATION 
        1. 
*DATABASE_BINARY_D3PLOT
LS-DYNA 
The Next Step 
$ 
$---------------  define model geometry and material parameters ---------------- 
$ 
*PART 
aluminum block 
         1         1         1 
*SECTION_SOLID 
         1 
*MAT_ELASTIC 
         1     2700.   70.e+09        .3 
*NODE 
       1              0.              0.              0.       7       7 
       2              1.              0.              0.       5       0 
       3              1.              1.              0.       3       0 
       4              0.              1.              0.       6       0 
       5              0.              0.              1.       4       0 
       6              1.              0.              1.       2       0 
       7              1.              1.              1.       0       0 
       8              0.              1.              1.       1       0 
*ELEMENT_SOLID 
       1       1       1       2       3       4       5       6       7       8 
$ 
$----------------  define boundary conditions and load curves ------------------ 
$ 
*LOAD_SEGMENT 
         1        1.        0.         5         6         7         8 
*DEFINE_CURVE 
         1 
                  0.                  0. 
                  1.             70.e+05
LS-DYNA 
The Next Step 
4.3  Heat Transfer Analysis (problem th01.k) 
LS-DYNA can solve steady state and transient heat transfer problems. Steady state problems are 
solved in one step, while transient problems are solved using an implicit method. Our 1-element 
problem will now be re-defined as a transient heat transfer problem as shown below: 
Q = 2.43e+07 W / m3 
1m
Aluminum 1100-O 
density  
modulus of elasticity   
Poisson Ratio   
coefficient of expansion 
heat capacity 
thermal conductivity   
2700 kg/m3 
70.e+09 Pa 
0.3 
23.6e-06 m/m K 
900 J/kg K 
220 W/m K 
We will solve for the temperature response of the cube as the result of internal heat generation, Q. 
All the surfaces of the cube are perfectly insulated. Therefore, all the heat generation goes into 
increasing the internal energy of the cube. The temperature response of the cube calculated by LS-
DYNA is shown in the figure below. The analytical solution is shown in the box.  
T =
Qt
ρVcp
T =
) t( )
(
2.43e + 07
(2700.)(1)(900.)
T = 10t
The keyword input for this problem is shown below. Important things to note are: 
•  The default initial condition is T=0 for all nodes. 
•  The default thermal boundary condition is adiabatic (i.e. perfectly insulted). Therefore, no 
thermal boundary conditions need be specified for this problem. 
•  The *CONTROL_SOLUTION keyword is used to specify this problem as thermal only. 
•  The entry on the *PART keyword points to the definition of thermal property data
LS-DYNA 
The Next Step 
Example 4-3 Aluminum cube transient heat transfer analysis (file: th01.k) 
set printing interval 
set thermal time step size 
specify as transient solution
specify heat transfer solution
*KEYWORD 
*TITLE 
th01.k – heat transfer – problem 1 
$ 
$------------------------ thermal solution keywords ---------------------------- 
$ 
*CONTROL_SOLUTION 
         1 
*CONTROL_THERMAL_SOLVER 
         1 
*CONTROL_THERMAL_TIMESTEP 
         0        1.        .1 
*DATABASE_TPRINT 
        .1 
$ 
$---------------  define solution control and output parameters ---------------- 
$ 
*CONTROL_TERMINATION 
        1. 
*DATABASE_BINARY_D3PLOT 
        .1 
$ 
$---------------  define model geometry and material parameters ---------------- 
$ 
*PART 
aluminum block 
         1         1                                                           1 
*SECTION_SOLID 
         1 
*MAT_THERMAL_ISOTROPIC 
         1     2700.         0  2.43e+07 
      904.      222. 
*NODE 
       1              0.              0.              0.       7       7 
       2              1.              0.              0.       5       0 
       3              1.              1.              0.       3       0 
       4              0.              1.              0.       6       0 
       5              0.              0.              1.       4       0 
       6              1.              0.              1.       2       0 
       7              1.              1.              1.       0       0 
       8              0.              1.              1.       1       0 
*ELEMENT_SOLID 
       1       1       1       2       3       4       5       6       7       8 
*END
LS-DYNA 
The Next Step 
4.4  Coupled thermal-stress analysis (problem cp01.k) 
In this problem, the cube is allowed to expand due to the temperature increase from internal heat 
generation. Keywords from the mechanical problem defined in section 4.1 and the thermal problem 
defined in section 4.3 are combined to define this thermal-stress problem. The keyword 
*MAT_ELASTIC_PLASTIC_THERMAL is used to define a material with a thermal coefficient of 
expansion. For this problem, α =23.6-06 m/m C. The aluminum blocks starts out at 0C (the default 
initial condition) and heats up 10C over the 1 second time interval . The x 
displacement of node 7 versus temperature increase as calculated by LS-DYNA is shown in the 
figure below. The curve is not smooth due to numerical noise in the solution because we are only 
using 1 element. The analytical solution is shown in the box. 
∆x = α∆T
= 23.6e − 06
(
)
) 10(
= 23.6e − 05
The keyword input for this problem is shown below. Important things to note are: 
•  *CONTROL_SOLUTION is set to 2. This defines the problem as a coupled thermal stress 
analysis.  
•  Defining both mechanical and thermal properties. 
•  Using a mechanical constitutive model (*MAT_ELASTIC_PLASTIC_THERMAL) that allows 
entry of a thermal coefficient of expansion and mechanical properties that are a function of 
temperature.  
•  The mechanical and thermal time steps are independent. For this problem, we are using the 
default explicit mechanical time step calculated by the code and have specified a thermal time
LS-DYNA 
The Next Step 
Example 4-4 Aluminum cube coupled thermal-stress solution (file: cp01.k) 
specify thermal-stress solution 
*KEYWORD 
*TITLE 
cp01.k - coupled thermal stress analysis - problem 1 
$ 
$---------------  define solution control and output parameters ---------------- 
$ 
*CONTROL_SOLUTION 
         2 
*CONTROL_TERMINATION 
        1. 
*DATABASE_BINARY_D3PLOT 
        .1 
$ 
$------------------------ thermal solution keywords ---------------------------- 
$ 
*CONTROL_THERMAL_SOLVER 
         1 
*CONTROL_THERMAL_TIMESTEP 
         0        1.        .1 
*DATABASE_TPRINT 
        .1 
$ 
$---------------  define model geometry and material parameters ---------------- 
$ 
*PART 
aluminum block 
         1         1         1                                                 1 
*SECTION_SOLID 
         1 
*MAT_ELASTIC_PLASTIC_THERMAL 
         1     2700. 
        0.      100. 
   70.e+09   70.e+09 
        .3        .3 
  23.6e-06  23.6e-06 
specify mechanical 
material 
specify thermal 
material 
*MAT_THERMAL_ISOTROPIC 
         1     2700.         0  2.44e+07 
      904.      222. 
*NODE 
       1              0.              0.              0.       7       7 
       2              1.              0.              0.       5       0 
       3              1.              1.              0.       3       0 
       4              0.              1.              0.       6       0 
       5              0.              0.              1.       4       0 
       6              1.              0.              1.       2       0 
       7              1.              1.              1.       0       0 
       8              0.              1.              1.       1       0 
*ELEMENT_SOLID 
       1       1       1       2       3       4       5       6       7       8