Most of the materials used in explicit dynamics require data table input. A data table is a series of constants that are interpreted when they are used. Data tables are always associated with a material number and are most often used to define nonlinear material data (stress-strain curves). The form of the data table (referred to as the TB table) depends upon the data being defined.
Wherever "load curve ID" is mentioned as required input, you actually input a material data curve ID. Material data curves are defined with the EDCURVE command.
MP,DENS - density
MP,EX - elastic modulus (default = 30e6)
MP,NUXY - Poisson's ratio (default = .3)
Orthotropic Elastic - Orthotropic material model. Use the MP command to input the required values.
MP,DENS - density
MP,EX - elastic moduli (also EY, EZ); one
value required
MP,NUXY - Minor Poisson's ratio (also
NUYZ, NUXZ); one value required
MP,PRXY - Major Poisson's ratio (also
PRXZ, PRYZ); one value required
MP,GXY - shear moduli (also GYZ and
GXZ); one value required
Note-If only one value is specified for a given material property family (i.e., EX), the other values will be automatically defined (e.g., EY = EZ = EX).
Anisotropic Elastic - This material description requires the full elasticity matrix. Because of symmetry, 21 constants are required.
Input density with MP. The constants are input in upper triangular form by means of the TB,ANEL command. To specify a material orientation axis, use the EDLCS and EDMP,ORTHO commands.
MP,DENS - density
TB,ANEL,
TBDATA, 1, C11, C12, C22, C13, C23,
C33
TBDATA, 7, C14, C24, C34, C44, C15,
C25
TBDATA, 13, C35, C45, C55, C16,
C26, C36
TBDATA, 19, C46, C56, C66
G is the shear modulus, V is the relative volume, 
is the Poisson's ratio, Cij is
the right Cauchy-Green strain tensor, and 
ij is the Kronecker delta. This option
is invoked when the shear modulus is the only material property defined. Input
the shear modulus using MP,GXY,,value.
Mooney-Rivlin Rubber - Incompressible rubber material model; nearly
identical to the 2-parameter existing ANSYS Mooney-Rivlin model. The strain
energy density function is defined in terms of input parameters C10, C01 and :
Input Poisson's ratio, , and density with MP, and the Mooney-Rivlin constants with TB and TBDATA. Data at only one temperature is
permitted and must be specified in locations 1 and 2 for the data table:
TB,MOONEY,
TBDATA, 1, C10
TBDATA, 2, C01 .
Viscoelastic - Linear viscoelastic material model introduced by Hermann and Peterson. The model assumes the deviatoric behavior:
where the shear relaxation modulus is given by:
(t) = G
+ (G0 - G) e-
t .
In the model, elastic bulk behavior, K, is assumed when calculating the
integrated pressure from the volume, V: p = K ln V. The parameters G , G0 ,
K and are required to define the linear viscoelastic material model. Input
these values with TB,EVISC and locations
46, 47, 48, and 61 of the TBDATA
command:
TB, EVISC
TBDATA, 46, G0
TBDATA, 47, G
TBDATA, 48, K
TBDATA, 61, 1/.
Note-For this material option, you must specify density [MP,DENS,,value].
TB, BISO
TBDATA, 1, 
Y (yield stress)
TBDATA, 2, Etan (tangent modulus)
Bilinear Kinematic (Plastic Kinematic, strain rate independent) - Classical bilinear kinematic hardening model that uses two slopes (elastic and plastic) to represent the stress-strain behavior of a material. The stress-strain behavior can be specified at only one temperature. Input elastic modulus (Exx), density (DENS), and Poisson's ratio (NUXY) with the MP command. Input the yield strength and tangent slope with TB,BKIN and locations 1 and 2 of the TBDATA command:
TB, BKIN
TBDATA, 1, Y (yield stress)
TBDATA, 2, Etan (tangent modulus)
Plastic Kinematic (strain rate dependent) - Isotropic, kinematic, or a
combination of isotropic and kinematic hardening models with strain rate
dependency and failure. Isotropic and kinematic contributions may be varied by
adjusting the hardening parameter between 0 (kinematic hardening only) and
1 (isotropic hardening only). Strain rate is accounted for using the
Cowper-Symonds model which scales the yield stress by the strain rate
dependent factor as shown below:
where 0 is the initial yield stress, 
is the strain rate, C and P are the
Cowper-Symonds strain rate parameters, 
peff is the effective plastic strain,
and Ep is the plastic hardening modulus which is given by Etan E / (E - Etan) .
The stress-strain behavior can only be specified at one temperature. Input the
elastic modulus (Exx), density (DENS), and Poisson's ratio (NUXY) with the MP command. Input the yield stress, tangent
slope, hardening parameter, strain rate parameters P and C, and the failure
strain with TB,PLAW,,,,1 and locations 1 - 6
of the TBDATA command:
TB, PLAW,,,,1
TBDATA, 1, Etan (tangent modulus)
TBDATA, 2, Y (yield stress)
TBDATA, 3, (hardening parameter)
TBDATA, 4, C (strain rate parameter)
TBDATA, 5, P (strain rate parameter)
TBDATA, 6, f (failure strain)
Power Law Plasticity - Strain rate dependent plasticity model typically used for metal and plastic forming analyses. Elastoplastic behavior with isotropic hardening is provided with this model. The material model has a powerlaw constitutive relationship which includes the Cowper-Symonds multiplier to account for strain rate:
where is the strain rate, C and P are the Cowper-Symonds strain rate
parameters, e is the elastic strain to yield, peff is the effective plastic strain, k
is the strength coefficient, and n is the hardening coefficient. The stress-strain
behavior can be specified at only one temperature. Input the elastic modulus
(Exx), density (DENS), and Poisson's ratio (NUXY) with the MP command. Input the strength coefficient,
hardening coefficient, and strain rate parameters P and C with TB,PLAW,,,,2 and locations 1 - 4 of the TBDATA command:
TB, PLAW,,,,2
TBDATA, 1, k (strength coefficient)
TBDATA, 2, n (hardening coefficient)
TBDATA, 3, C (strain rate parameter)
TBDATA, 4, P (strain rate parameter)
3-Parameter Barlat - Anisotropic plasticity model developed by Barlat and Lian3 used for modeling sheets under plane stress conditions. Both exponential and linear hardening rules are available. The anisotropic yield criterion for plane stress is defined as:
2Ym = a|K1+K2|m + a|K1-K2|m + c|2K2|m
where Y is the yield stress, a and c are anisotropic material constants, m is
Barlat exponent, and K1 and K2 are defined by:
where h and p are additional anisotropic material constants. For the exponential hardening option, the material yield strength is given by:
Y = k (0 + p)n
where k is the strength coefficient, 0 is the initial strain at yield, p is the
plastic strain, and n is the hardening coefficient. All of the anisotropic material
constants, excluding p which is determined implicitly, are determined from
Barlat and Lian width to thickness ratio (R) values as shown:
c = 2 - a
The width to thickness ratio for any angle 
can be calculated from:
Above, is the uniaxial tension in the direction. The stress-strain behavior
can be specified at only one temperature. Input the elastic modulus (Exx),
density (DENS), and Poisson's ratio (NUXY) with the MP command. Input the hardening rule type
HR : equal to 1 for linear or 2 for exponential,: tangent modulus for HR = 1 or
strength coefficient for HR = 2,: yields stress for HR = 1 or hardening coefficient
for HR = 2, the Barlat exponent m, and the width to thickness ratio values R00,
R45, and R90 with TB,PLAW,,,,3 and locations
1 - 7 of the TBDATA command:
TB, PLAW,,,,3
TBDATA, 1, HR (hardening rule type)
TBDATA, 2, Etan or k (tangent modulus
or strength coefficient)
TBDATA, 3, Y or n (yield stress or
hardening coefficient)
TBDATA, 4, m (Barlat exponent)
TBDATA, 5, R00
TBDATA, 6, R45
TBDATA, 7, R90
Rate Sensitive Powerlaw Plasticity - Strain rate dependent plasticity model typically used for superplastic forming analyses. The material model follows a Ramburgh - Osgood constitutive relationship of the form:
yy = kmn
where is the strain, is the strain rate, k is the material constant, m is the
hardening coefficient, and n is the strain rate sensitivity coefficient. The
stress-strain behavior can be specified at only one temperature. Input the
elastic modulus (Exx), density (DENS), and Poisson's ratio (NUXY) with the MP command. Input the material constant,
hardening coefficient, strain rate sensitivity coefficient, and and initial strain rate
with TB,PLAW,,,,4 and locations 1 - 4 of the
TBDATA command:
TB, PLAW,,,,4
TBDATA, 1, k (material constant)
TBDATA, 2, m (hardening coefficient)
TBDATA, 3, n (strain rate parameter)
TBDATA, 4, 
(initial strain rate)
Strain Rate Dependent Plasticity - Strain rate dependent isotropic plasticity model used mainly for metal and plastic forming analyses.
In this model, a load curve is used to describe the initial yield strength, 0, as a
function of effective strain rate. The yield stress for this material model is
defined as:
where 0 is the initial yield strength, 
is the effective strain rate, peff is the
effective plastic strain, and Eh is given by:
The stress-strain behavior can be specified at only one temperature. Input the elastic modulus (Exx), density (DENS), and Poisson's ratio (NUXY) using the MP command. Input the load curve ID for defining the initial yield stress vs effective strain rate, the tangent modulus, the load curve ID for defining the elastic modulus vs effective strain rate (optional), the load curve ID for defining the tangent modulus vs effective strain rate (optional), and the load curve ID for defining the von Mises stress at failure vs effective strain rate using TB,PLAW,,,,5 and locations 1 - 5 of the TBDATA command:
TB, PLAW,,,,5
TBDATA, 1, LCID1 (load curve ID for
defining the initial yield stress vs effective strain rate)
TBDATA, 2, Etan (hardening coefficient)
TBDATA, 3, LCID2 (the load curve ID
for defining the elastic modulus vs effective strain rate)
TBDATA, 4, LCID3 ( the load curve ID
for defining the tangent modulus vs effective strain rate)
TBDATA, 5, LCID4 (the load curve ID
for defining von Mises stress at failure vs effective strain rate).
Barlat Anisotropic Plasticity - Anisotropic plasticity model developed by
Barlat, Lege, and Brem4 used for modeling material behavior in forming
processes. The anisotropic yield function is defined as:
= |S1 - S2|m + |S2 - S3|m + |S3 - S1|m
where m is the flow potential exponent and Si are the principal values of the symmetric matrix Sij.
Sxx = 
[ c(xx - yy) - b(zz - xx)]
Syy = [ a(yy - zz) - c(xx - yy)]
Szz = [ b(zz - xx) - a(yy - zz)]
Syz = f yz
Szx = g zx
Syz = h xy.
where a, b, c, f, g, and h represent the anisotropic material constants. When a=b=c=f=g=h=1, isotropic material behavior is modeled and the yield surface reduces to the Tresca surface for m = 1 and the von Mises surface for m = 2 or 4. For this material option, the yield strength is given by:
Y = k (1 + 0)n
where k is the strength coefficient, 0 is the initial strain at yield, and n is the
hardening coefficient. The stress-strain behavior can be specified at only one
temperature.
Input the elastic modulus (Exx), density (DENS), and Poisson's ratio (NUXY) with the MP command. Input the strength coefficient, the initial strain at yield, the hardening coefficient, the flow potential exponent, and the Barlat anisotropic constants a-h with TB,PLAW,,,,6 and locations 1 - 10 of the TBDATA command:
TB, PLAW,,,,6
TBDATA, 1, k (strength coefficient)
TBDATA, 2, 0 (initial strain)
TBDATA, 3, n (hardening coefficient)
TBDATA, 4, m (flow potential (Barlat)
exponent)
TBDATA, 5, a
TBDATA, 6, b
TBDATA, 7, c
TBDATA, 8, f
TBDATA, 9, g
TBDATA, 10, h
Transversely Anisotropic Elastic Plastic - Fully iterative anisotropic plasticity model available for shell elements only. In this model the yield function given by Hill5 is defined as:
F() 
where R is the anisotropic hardening parameter which is the ratio of the
in-plane plastic strain rate, 
, to the out of plane plastic strain rate, 
:
R = 
The stress-strain behavior can be specified at only one temperature. Input the elastic modulus (Exx), density (DENS), and Poisson's ratio (NUXY) with the MP command. Input the strength coefficient, the initial strain at yield, the yield stress, tangent modulus, anisotropic hardening parameter, and a load curve ID for yield stress versus plastic strain with TB,PLAW,,,,7 and locations 1 - 4 of the TBDATA command:
TB, PLAW,,,,7
TBDATA, 1, Y (yield stress)
TBDATA, 2, Etan (tangent modulus)
TBDATA, 3, R (anisotropic hardening
parameter)
TBDATA, 4, LCID (Load curve ID for
yield stress vs plastic strain).
Piecewise Linear Plasticity - An elastic-plastic material option that allows stress vs. strain curve input and strain rate dependency. Failure can also be modeled with the material based on plastic strain. Strain rate may be accounted for using the Cowper-Symonds model, which scales the yield stress as shown:
where 0 is the yield at constant rate, 
is the effective strain rate, and C and P
are strain rate parameters.
Input the elastic modulus (Exx), density (DENS), and Poisson's ratio (NUXY) with the MP command. Input the yield stress, the tangent modulus, the failure strain, the strain rate parameter C, the strain rate parameter P, the load curve ID for defining effective stress vs plastic strain, and the load curve ID for defining strain rate scaling with TB,PLAW,,,,8 and locations 1 - 7 of the TBDATA command:
TB, PLAW,,,,8
TBDATA, 1, Y
TBDATA, 2, Etan (hardening coefficient)
TBDATA, 3, F
TBDATA, 4, C
TBDATA, 5, P
TBDATA,6, LCID 1
TBDATA,7, LCID 2
ij = ijsk + ij [po
/ (1+-)]
where ijsk is the skeletal stress, po is the initial foam pressure, is the ratio of
foam to polymer density, ij is the Kronecker delta, and is the volumetric
strain which is defined by:
= V - 1 + o,
where V is the relative volume and o is the initial volumetric strain. The yield
condition is applied to the principal trial stresses and is defined by:
Y = a + b(1 + c),
where a, b, and c are user defined input constants. The stress-strain behavior can be specified at only one temperature. Input the elastic modulus (Exx) and density (DENS) with the MP command. Poisson's ratio for this model is assumed to be zero. Input the yield stress constants a, b, and c, the initial foam pressure, the ratio of foam to polymer density, and the initial volumetric strain with TB,FOAM,,,,1 and locations 1 - 6 of the TBDATA command:
TB, FOAM,,,,1
TBDATA, 1, a
TBDATA, 2, b
TBDATA, 3, c
TBDATA, 4, po (initial foam pressure)
TBDATA, 5, (ratio of foam to polymer
density)
TBDATA, 6, o (initial volumetric strain).
Low Density Foam - Highly compressible (urethane) foam material model
often used for padded materials such as seat cushions. In compression, the
model assumes hysteresis unloading behavior with possible energy dissipation.
In tension the material model behaves linearly until tearing occurs. For uniaxial
loading, the model assumes that there is no coupling in transverse directions.
By using input shape factor controls (a hysteresis unloading factor (HU), a
decay constant (), and a shape factor for unloading) the observed unloading
behavior of foams can be closely approximated. The stress-strain behavior
can be specified at only one temperature. Input the elastic modulus (Exx) and
density (DENS) with the MP command.
Input the load curve ID for stress vs strain, the tension cut off (tearing) stress,
the hysteresis unloading factor, the decay constant, the shape factor for
unloading, the failure option when cut off stress is reached, and the bulk
viscosity action flag with TB,FOAM,,,,2 and
locations 1 - 8 of the TBDATA
command:
TB, FOAM,,,,2
TBDATA, 1, LCID (load curve ID for
stress-strain behavior)
TBDATA, 2, TC (tension cutoff stress,
default=1E20)
TBDATA, 3, HU (hyperelastic unloading
factor: between 1.0 - no energy dissipation and 0.0 - full energy dissipation)
TBDATA, 4, (decay constant)
TBDATA, 5, DAMP (viscous coefficient,
values between 0.05 and 0.5 are recommended)
TBDATA, 6, SHAPE (shape unloading
factor, default=1)
TBDATA, 7, FAIL (failure option when
cut off stress is reached: 0.0 - tensile stress remains at cut off value, 1.0 -
tensile stress reset to zero)
TBDATA, 8, BVFLAG (bulk viscosity
action flag: 0.0 - no bulk viscosity and 1.0 - bulk viscosity active)
Viscous Foam - Energy absorbing foam material used in crash-simulation models. The model consists of a nonlinear elastic stiffness in parallel with a viscous damper. The elastic stiffness is intended to limit total crush while the viscosity absorbs energy. The elastic stiffness, E', and initial viscous coefficient, V', are both nonlinear functions of the relative volume, V:
where E1 is the initial elastic stiffness, V2 is the initial viscous coefficient, and n1 and n2 are the powerlaws for the elastic stiffness and viscous coefficient. The stress-strain behavior can be specified at only one temperature. Input the initial elastic stiffness (Exx), Poisson's ratio (NUXY), and density (DENS) with the MP command. Input the powerlaw for the elastic stiffness, the initial viscous coefficient, the elastic stiffness for viscosity (required to prevent timestep problems), and the powerlaw for viscosity with TB,FOAM,,,,3 and locations 1 - 4 of the TBDATA command:
TB, FOAM,,,,3
TBDATA, 1, n1 (powerlaw for the elastic
stiffness)
TBDATA, 2, V2 (initial viscous
coefficient)
TBDATA, 3, E1 (elastic stiffness for
viscosity)
TBDATA, 4, n2 (powerlaw for the
viscous coefficient)
Crushable Foam - Material model used for crushable foams in side impact and other applications where cyclic behavior is unimportant. The foam model is strain rate dependent and crushes one-dimensionally with a Poisson's ratio that is essentially zero. In the formulation, the elastic modulus is considered constant and the stress is updated assuming elastic behavior:
ijn+1 = ijn + E ijn+1/2 
tn+1/2 ,
where ij is the strain rate, E is the elastic modulus, and t is time. The model
includes a tensile stress cutoff value which defines failure under tensile loads.
For stresses below the tensile cut off value the model predicts similar response
between tensile and compressive loading. It is important to have a nonzero
value for the cutoff stress to prevent deterioration of the material under small
tensile loads. Input the elastic modulus (Exx), density (DENS), and Poisson's
ratio (NUXY) with the MP command. Input
the load curve ID for defining stress vs volumetric strain, the tension cutoff
value, and the viscous damping coefficient with TB,FOAM,,,,4 and locations 1 - 3 of the TBDATA command:
TB, FOAM,,,,4
TBDATA, 1, LCID (load curve ID for
defining yield stress vs volumetric strain)
TBDATA, 2, TC (tension cutoff value)
TBDATA, 3, DAMP (viscous damping
coefficient, values between 0.05 and 0.5 are recommended)
Honeycomb - Orthotropic material model used for honeycomb materials. The behavior of the model before compaction is orthotropic where the components of the stress tensor are uncoupled. The elastic moduli are considered to vary linearly with relative volume as shown below:
where
and
V = the relative volume (defined as ratio of current to original volume)
Vf = fully compacted volume.
Load curves can be used to input the magnitude of the average stress as the relative volume changes. Each curve must have the same abscissa values. Curves can be defined either as a function or relative volume or volumetric strain (1 - V). Input the elastic modulus (Exx), density (DENS), and Poisson's ratio (NUXY) with the MP command. Input all values shown below with TB,HONEY and locations 1 - 17 of the TBDATA command:
TB,HONEY
TBDATA, 1, Y (yield stress for fully
compacted honeycomb)
TBDATA, 2, Vf (volume of fully
compacted honeycomb)
TBDATA, 3, 
(material viscosity
coefficient)
TBDATA, 4, Eaau (Elastic modulus in aa
direction for uncompressed configuration)
TBDATA, 5, Ebbu (Elastic modulus in bb
direction for uncompressed configuration)
TBDATA, 6, Eccu (Elastic modulus in cc
direction for uncompressed configuration)
TBDATA, 7, Gabu (Shear modulus in ab
direction for uncompressed configuration)
TBDATA, 8, Gcbu (Shear modulus in cb
direction for uncompressed configuration)
TBDATA, 9, Gcau (Shear modulus in ca
direction for uncompressed configuration)
TBDATA, 10, LCA (Load curve ID for aa
direction stress vs relative volume or volumetric strain)
TBDATA, 11, LCB (Load curve ID for bb
direction stress vs relative volume or volumetric strain)
TBDATA, 12, LCC (Load curve ID for cc
direction stress vs relative volume or volumetric strain)
TBDATA, 13, LCS (Load curve ID for
shear yield vs relative volume or volumetric strain)
TBDATA, 14, LCAB (Load curve ID for
ab direction stress vs relative volume or volumetric strain)
TBDATA, 15, LCBC (Load curve ID for
bc direction stress vs relative volume or volumetric strain)
TBDATA, 16, LCCA (Load curve ID for
ca direction stress vs relative volume or volumetric strain)
TBDATA, 17, LCRS (Load curve ID for
strain rate effects. This input is optional. The curves defined above are scaled
using this curve.)
= nonlinear shear stress parameter.
TB,COMPOSITE
TBDATA, 1, KFAIL (bulk modulus of
material in compressive failure)
TBDATA, 2, S12 (shear strength)
TBDATA, 3, S1 (longitudinal tensile
stress)
TBDATA, 4, S2 (transverse tensile
strength)
TBDATA, 5, C2 (transverse
compressive strength)
TBDATA, 6, (nonlinear shear stress
parameter).
Johnson and Cook express the flow stress as
where:
A, B, C, n, and m are material constants,
is effective plastic strain
is effective plastic strain rate for 
T* = homologous temperature = 
The strain at fracture is given by:
Where 
is the ratio of pressure divided by effective stress:
Fracture occurs when the damage parameter
reaches the value of 1.
Input the Young's modulus (EX), density (DENS), and Poisson's ratio (NUXY) with the MP command. Input the parameters described in the above equations with TB,EOS and locations 1 - 15 of the TBDATA command:
TB,EOS,,,,1,EOSOPT
TBDATA, 1, (ALPHA)
TBDATA, 2, B
TBDATA, 3, (NU)
TBDATA, 4, C
TBDATA, 5, M
TBDATA, 6, Tmelt
TBDATA, 7, Troom
TBDATA, 8,
TBDATA, 9, CP (specific heat)
TBDATA, 10, pressure cut-off
TBDATA, 11, D1
TBDATA, 12, D2
TBDATA, 13, D3
TBDATA, 14, D4
TBDATA, 15, D5
When using the Johnson-Cook Plasticity Model, you can define either of two types of equations of state: Linear Polynomial (EOSOPT=1) and Gruneisen (EOSOPT=2). Each has its own set of required constants that are input in positions 16+ of the TBDATA command.
Linear Polynomial (EOSOPT=1): This equation of state is linear in internal energy. The pressure is given by:
where terms 
and 
are set to zero if 
and 
is the
ratio of current density to initial density. Input the required constants with
positions 16+ of the TBDATA
command:
TBDATA, 16, C0
TBDATA, 17, C1
TBDATA, 18, C2
TBDATA, 19, C3
TBDATA, 20, C4
TBDATA, 21, C5
TBDATA, 22, C6
TBDATA, 23, E0 (initial internal energy)
TBDATA, 24, V0 (initial relative volume)
Gruneisen (EOSOPT=2): This equation of state defines the pressure volume relationship in one of two ways, depending on whether the material is compressed or expanded.
The Gruneisen equation of state with cubic shock velocity-particle velocity defines pressure for compressed materials as:
and for expanded materials as:
where C is the intercept of the vs-vp curve; S1, S2, and S3 are the coefficients
of the slope of the vs-vp curve, 
is the Gruneisen gamma, a is the first order
volume correction to , and 
Input the required constants with positions 16+ of the TBDATA command:
TBDATA, 16, C
TBDATA, 17, S1
TBDATA, 18, S2
TBDATA, 19, S3
TBDATA, 20, 0
TBDATA, 21, A
TBDATA, 22, E0 (initial relative energy)
TBDATA, 23, V0 (initial relative volume)
Null Material - This material allows equations of state to be considered without computing deviatoric stresses. Optionally, you can define a viscosity. Erosion in tension and compression is possible. The Young's modulus and Poisson's ratio are used only for setting the contact interface stiffness, so you should use reasonable values.
Input the Young's modulus (EX), density (DENS), and Poisson's ratio (NUXY) with the MP command. Input the parameters described in the above equations with TB,EOS and locations 1 - 15 of the TBDATA command:
TB,EOS,,,,2,EOSOPT
TBDATA, 1, Pressure Cutoff
TBDATA, 2, Viscosity Coefficient
TBDATA, 3, Relative volume for erosion
in tension
TBDATA, 4, Relative volume for erosion
in compression
When using the Null Model, you can define either of two types of equations of state: Linear Polynomial (EOSOPT=1) and Gruneisen (EOSOPT=2). Each has its own set of required constants that are input in positions 16+ of the TBDATA command. See the descriptions of these two equations of state under the Johnson-Cook Plasticity Model, above.
Along with the EDMP command, you must use the MP command to specify Young's modulus (Ex), Poisson's ratio (NUXY), and density (DENS) for the rigid body's material type. Realistic material property values are required so that the stiffness of the contact surfaces can be calculated by the program. For this reason, never use unrealistically high values of Young's modulus or density for a rigid body in an explicit dynamic analysis. A rigid body cannot be stiffened because it is perfectly rigid.
Because the motion of the mass center of a rigid body is transferred to its nodes, constraints should not be applied to rigid bodies using the D command. The constraints and initial velocities of one node of a rigid body will be transferred to the center of mass of the body. However, if more than one node is constrained, it is hard to determine which constraints will be used. To properly apply constraints to a rigid body, the translational (VAL1) and rotational (VAL2) constraint parameter fields of the EDMP command are used as shown below:
VAL1 Translational constraint parameter (relative to global Cartesian coordinates).
Cable - Use this model to realistically model elastic cables. No force will develop in compression. The force, F, generated by the cable is nonzero if and only if the cable is in tension. The force is given by:
where L is the change in length
L = current length - (initial length - offset)
and the stiffness is defined as:
The area and offset are defined by means of the real constants for LINK167. For a slack cable, the offset should be a negative length. For an initial tensile force, the offset should be positive. If a load curve is specified, Young's modulus is ignored and the load curve is used instead. The points on the load curve are defined as engineering stress versus engineering strain, i.e., the change in length over the initial length.
Use the MP and EDMP commands to input the required values:
MP,DENS
MP,EX
EDMP,CABLE,MAT,Load Curve ID