TB, Lab
, MATID
,
NTEMP
, NPTS
,
TBOPT
, EOSOPT
,
FuncName
Activates a data table for material
properties or special element input.
For a list of elements and the material models they
support (Lab
value), see Element Support for Material Models in the Element Reference.
For a list of material models and the elements that support them, see Material Model Element Support in the Material Reference.
Lab
Material model data table type:
AFDM  —  
AHYPER  —  
ANEL  —  
BB  —  
BH  —  Magnetic field data. 
BISO  —  Bilinear isotropic hardening using von Mises or Hill plasticity. 
BKIN  —  Bilinear kinematic hardening using von Mises or Hill plasticity. 
CAST  —  
CDM  —  Mullins effect (for isotropic hyperelasticity models). 
CGCR  —  Crackgrowth fracture criterion (CGROW). 
CHABOCHE  —  Chaboche nonlinear kinematic hardening using von Mises or Hill plasticity. 
COMP  —  Composite damage (explicit dynamic analysis). 
CONCR  —  Concrete element or material data. 
CREEP  —  Creep. Pure creep, creep with isotropic hardening plasticity, or creep with kinematic hardening plasticity using both von Mises or Hill potentials. 
CTE  —  Secant coefficient of thermal expansion. 
CZM  —  
DENS  —  
DISCRETE  —  Explicit springdamper (discrete). 
DMGE  —  
DMGI  —  
DP  —  
DPER  —  
EDP  —  Extended DruckerPrager (for granular materials such as rock, concrete, soil, ceramics and other pressuredependent materials). 
ELASTIC  —  Elasticity. For full harmonic analyses, properties can be defined as frequency or temperaturedependent (TBFIELD). 
EOS  —  Equation of state (explicit dynamic analysis). 
EVISC  —  Viscoelastic element data (explicit dynamic analysis). 
EXPE  —  
FCON  —  Fluid conductance data (explicit dynamic analysis). 
FCLI  —  Material strength limits for calculating failure criteria. 
FLUID  —  
FOAM  —  Foam (explicit dynamic analysis). 
FRIC  —  Coefficient of friction based on Coulomb's Law or userdefined friction. 
GASKET  —  
GCAP  —  Geological cap (explicit dynamic analysis). 
GURSON  —  Gurson pressuredependent plasticity for porous metals. 
HFLM  —  
HILL  —  Hill anisotropy. When combined with other material options, simulates plasticity, viscoplasticity, and creep  all with the Hill potential. 
HONEY  —  Honeycomb (explicit dynamic analysis). 
HYPER  —  Hyperelasticity material models (ArrudaBoyce, BlatzKo, Extended Tube, Gent, MooneyRivlin [default], NeoHookean, Ogden, Ogden Foam, Polynomial Form, Response Function, Yeoh, and userdefined). 
INTER  —  
JOIN  —  Joint (linear and nonlinear elastic stiffness, linear and nonlinear damping, and frictional behavior). 
JROCK  —  
MC  —  
MIGR  —  
MOONEY  —  MooneyRivlin hyperelasticity (explicit dynamic analysis). 
MPLANE  —  
NLISO  —  Voce isotropic hardening law (or power law) for modeling nonlinear isotropic hardening using von Mises or Hill plasticity. 
PELAS  —  
PERF  —  
PIEZ  —  
PLASTIC  —  Nonlinear plasticity. 
PLAW  —  Plasticity laws (explicit dynamic analysis). 
PM  —  Porous media. Coupled porefluid diffusion and structural model of porous media. 
PRONY  —  Prony series constants for viscoelastic materials. 
PZRS  —  
RATE  —  Ratedependent plasticity (viscoplasticity) when combined with the BISO, NLISO or PLASTIC material options, or ratedependent anisotropic plasticity (anisotropic viscoplasticity) when combined with the HILL and BISO, NLISO or PLASTIC material options. The exponential viscohardening option includes an explicit function for directly defining static yield stresses of materials. The Anand unified plasticity option requires no combination with other material models. 
SDAMP  —  Material damping coefficients. 
SHIFT  —  Shift function for viscoelastic materials. 
SMA  —  Shape memory alloy for simulating hysteresis superelastic behavior with no performance degradation. Plane stress is not supported. 
SOIL  —  
STATE  — 
Userdefined state variables.
Valid with TB,USER and used with either the

SWELL  —  Swelling strain function. 
THERM  —  
UNIAXIAL  —  Uniaxial stressstrain relation associated with the Cast iron material model. 
USER  —  Userdefined material model (generalpurpose except for incompressible material models) or thermal material model. 
WEAR  — 
MATID
Material reference identification number. Default = 1.
NTEMP
The number of temperatures for which data will be provided (if applicable). Specify temperatures via the TBTEMP command.
NPTS
For most labels where NPTS
is defined, the number of data
points to be specified for a given temperature. Define data points via the
TBDATA or TBPT commands.
EOSOPT
Indicates which equation of state model will be used. Used only for explicit
dynamics, and only when Lab
= EOS.
1  —  Linear polynomial equation of state 
2  —  Gruneisen equation of state 
3  —  Tabulated equation of state 
FuncName
The name of the function to be used (entered as
%tabname
%, where tabname
is the
name of the table created by the Function Tool). Valid only when
Lab
= JOIN (joint element material) and nonlinear stiffness
or damping are specified on the TBOPT
field (see "JOIN  Joint Element Specifications"). The function must be previously defined using the Function
Tool. To learn more about how to create a function, see Using the Function Tool in the Basic Analysis Guide.
Following are input requirements (NTEMP
,
NPTS
, and TBOPT
values) and links to
detailed documentation for each data table type
(TB,Lab
value):
NTEMP:
Not used.
NPTS
:Not used.
TBOPT:
Acoustic material options:
Material properties
Thin layer
Rectangular crosssection
Circular crosssection
Defining Acoustic Material Properties in the Acoustic Analysis Guide.
Acoustic FrequencyDependent Materials in the Material Reference.
See the TBFIELD command for more information about defining temperature and/or frequencydependent properties.
NTEMP
:Number of temperatures for which data will be provided. Default = 1. Maximum = 40.
NPTS
:Number of data points to be specified for a given temperature.
TBOPT
:Anisotropic hyperelastic material options.
Polynomial strain energy potential.
Exponential strain energy potential.
Define the A vector.
Define the B vector.
Volumetric potential.
Anisotropic Hyperelasticity in the Material Reference.
Anisotropic Hyperelasticity in the Mechanical APDL Theory Reference
This material model is not supported for use with the coefficient of thermal expansion (TB,CTE).
NTEMP
:Number of temperatures for which data will be provided. Default = 6. Maximum = 6.
NTEMP
is not used for explicit dynamic elements.
NPTS
:Not used.
TBOPT
:Anisotropic elastic matrix options.
Elasticity matrix used as supplied (input in stiffness form).
Elasticity matrix inverted before use (input in flexibility form). This option is not valid for explicit dynamic elements.
NTEMP
:Number of temperatures for which data will be provided. Default = 1. The maximum
must be a value such that (NTEMP
x
NPTS
) <= 1000.
NPTS
:Number of material constants. If TBOPT
= ISO, then
NPTS
= 7. If TBOPT
= 1, then
NPTS
= 1.
TBOPT
:Isochoric or volumetric strainenergy function:
Define material constants for isochoric strain energy.
Define material constants for volumetric strain energy.
BergstromBoyce in the Mechanical APDL Theory Reference.
BergstromBoyce Material in the Material Reference.
BergstromBoyce Hyperviscoelastic Material Model in the Structural Analysis Guide.
NTEMP
:Not used.
NPTS
:Number of data points to be specified. Default = 20. Maximum = 500.
TBOPT
:Not used.
Magnetic Materials in the Material Reference.
Additional Guidelines for Defining Regional Material Properties and Real Constants in the LowFrequency Electromagnetic Analysis Guide.
NTEMP
:Number of temperatures for which data will be provided. Default = 1. Maximum = 6.
NPTS
:Not used.
TBOPT
:Not used.
Bilinear Isotropic Hardening in the Material Reference.
Nonlinear Inelastic Models in the ANSYS LSDYNA User's Guide.
NTEMP
: Number of temperatures for which data will be provided. Default = 1. Maximum = 6.
NPTS
: Not used.
TBOPT
: Stressstrain options (not used in an explicit dynamics analysis).
No stress relaxation with temperature increase (not recommended for nonisothermal problems).
Rice's hardening rule, which takes into account stress relaxation with increasing temperature (default).
Bilinear Kinematic Hardening in the Material Reference.
Nonlinear Inelastic Models in the ANSYS LSDYNA User's Guide.
NTEMP:
Number of temperatures for which data will be provided. Default = 1. Maximum = 10.
NPTS:
Not used.
TBOPT:
Defines hardening type.
Specifies cast iron plasticity with isotropic hardening.
Cast Iron in the Material Reference.
NTEMP
:Number of temperatures for which data will be provided. Default = 1. The maximum
must be a value such that (NTEMP
x
NPTS
) <= 1000.
NPTS
:Number of data points to be specified for a given temperature.
TBOPT
:Mullins effect option:
Pseudoelastic model with modified OgdenRoxburgh damage function.
Requires NPTS
= 3.
Mullins Effect in the Mechanical APDL Theory Reference.
Mullins Effect in the Material Reference.
Mullins Effect Material Model in the Structural Analysis Guide.
NTEMP
:Number of temperatures for which data will be provided. Default = 1.
NPTS
:Number of data points to be specified for a given temperature.
TBOPT
:Fracture criterion option:
Linear fracture criterion. Valid when NPTS
=
3.
Bilinear fracture criterion. Valid when NPTS
=
4.
BK fracture criterion. Valid when NPTS
=
3.
Modified BK (Reeder) fracture criterion. Valid when
NPTS
= 4.
Wu's Power Law fracture criterion. Valid when
NPTS
= 6.
Userdefined fracture criterion. Valid when
NPTS
= 20.
Circumferential stress criterion based on when sweeping around the crack tip at a given radius. Valid
when NPTS
= 1. This option is used in an XFEMbased
crackgrowth analysis only.
Maximum circumferential stress criterion. Valid when
NPTS
= 1. This option is used in an XFEMbased
crackgrowth analysis only.
Rigid linear evolution law for the decay of stress. Valid when
NPTS
= 4. This option is used in an XFEMbased
crackgrowth analysis only.
Paris' Law for fatigue crack growth. Valid when
NPTS
= 2.
Note: In an XFEMbased crackgrowth analysis, the only valid options are PSMAX, STTMAX and RLIN. The PARIS option is valid for XFEMbased fatigue crackgrowth analysis only.
Fracture Criteria in the Structural Analysis Guide.
CGROW command in the Command Reference.
NTEMP
:Number of temperatures for which data will be provided. Default = 1. The maximum
value of NTEMP
is such that
NTEMP
x (1 + 2NPTS
) =
1000.
NPTS
:Number of kinematic models to be superposed. Default = 1. Maximum = 5.
TBOPT
:Not used.
NTEMP
:Number of temperatures for which data will be provided (used only if
TBOPT
= 0 or 1). Default = 6. Maximum = 6.
NPTS
:Not used.
TBOPT
:Concrete material options.
DruckerPrager concrete strength parameters.
Rankine tension failure parameter.
DruckerPrager concrete dilatation.
DruckerPrager concrete exponential hardening/softening/dilitation (HSD) behavior.
DruckerPrager concrete steel reinforcement HSD behavior.
DruckerPrager concrete fracture energy HSD behavior.
DruckerPrager concrete linear HSD behavior.
DruckerPrager concrete joint parameters.
DruckerPrager concrete joint tension cutoff.
DruckerPrager concrete joint orientation.
MenetreyWillam constitutive model.
General concrete option for element SOLID65.
Concrete damage model for explicit dynamic elements SOLID164 and SOLID168.
NTEMP
:Number of temperatures for which data will be provided. Default = 1. Maximum value
of NTEMP
is such that NTEMP
x
NPTS
= 250 for explicit creep. There is no limit for
implicit creep.
NPTS
:Number of data points to be specified for a given temperature. Default = 72 for explicit creep. There is no limit for implicit creep with the USER CREEP option.
TBOPT
:Creep model options.
(or Blank) Explicit creep option. Creep is defined by constants C_{6}, C_{12}, and C_{66}, via TBDATA. See Primary Explicit Creep Equation for C6 = 0 through Irradiation Induced Explicit Creep Equation for C66 = 5 for the associated equations. (Applicable to SOLID65.) C_{6} = 100 defines the USER CREEP option for explicit creep. You must define the creep law using the subroutine USERCR.F. See the Guide to UserProgrammable Features in the Mechanical APDL Programmer's Reference for more information.
Implicit creep option. See Table 4.2: Implicit Creep Equations for a list of available equations. Use TBTEMP and TBDATA to define temperaturedependent constants. (Applicable to LINK180 , SHELL181, PLANE182, PLANE183, SOLID185, SOLID186 , SOLID187 , BEAM188, BEAM189, SOLSH190, SHELL208, SHELL209, REINF264, REINF265, SOLID272, SOLID273, SHELL281, SOLID285, PIPE288, PIPE289, and ELBOW290).
USER CREEP option (applicable to LINK180, SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, BEAM188, BEAM189, SOLSH190, SHELL208, SHELL209, REINF264, REINF265, SOLID272, SOLID273, SHELL281, SOLID285, PIPE288, PIPE289, and ELBOW290). You must define the creep law using the subroutine USERCREEP.F. See the Guide to UserProgrammable Features in the Mechanical APDL Programmer's Reference for more information. Use TBTEMP and TBDATA to define temperaturedependent constants. For implicit creep, use with TB,STATE for defining the number of state variables.
Creep in the Material Reference.
Creep in the Structural Analysis Guide.
See also Material Model Combinations.
NTEMP:
No limit.
NPTS:
Not used.
TBOPT:
Enter the secant coefficients of thermal expansion (CTEX,CTEY,CTEZ) (default).
Userdefined thermal strain. For more information, see Subroutine userthstrain (Defining Your Own Thermal Strain) in the Mechanical APDL Programmer's Reference.
Thermal Expansion in the Material Reference.
See also TBFIELD (for defining frequencydependent, temperaturedependent, and userdefined fieldvariablebased properties).
NTEMP
:Number of temperatures for which data will be provided. Default = 1.
NPTS
:Number of data points to be specified for a given temperature.
TBOPT
:Cohesive zone material options.
Exponential material behavior. Valid for interface elements and contact elements.
Bilinear material behavior. Valid for interface elements, contact elements, and in an XFEMbased crackgrowth analysis when cohesive behavior on the initial crack is desired.
Bilinear material behavior with linear softening characterized by maximum traction and maximum separation. Valid for contact elements only.
Bilinear material behavior with linear softening characterized by maximum traction and critical energy release rate. Valid for contact elements only.
Viscous regularization. Valid for interface elements and contact elements. Also valid in an XFEMbased crackgrowth analysis when cohesive behavior is specified for the initial crack.
Userdefined option. Valid for interface elements only.
Cohesive Zone Material (CZM) Model in the Mechanical APDL Theory Reference.
Cohesive Material Law in the Material Reference.
Subroutine userCZM (Defining Your Own Cohesive Zone Material) in the Programmer's Reference.
Crack Growth Simulation, Interface Delamination, and Fatigue Crack Growth in the Fracture Analysis Guide.
XFEMBased Crack Analysis and CrackGrowth Simulation in the Fracture Analysis Guide.
NTEMP
:Not used.
NPTS
:1
TBOPT
:Not used.
See the TBFIELD command and UserDefined Field Variables in the Mechanical APDL Material Reference and for more information about defining temperaturedependent and/or userdefined fieldvariablebased properties.
NTEMP
:Not used.
NPTS
:Not used.
TBOPT
:Explicit springdamper (discrete) material options.
Linear elastic spring (translational or rotational elastic spring) (default).
Linear viscous damper (linear translational or rotational damper)
Elastoplastic spring (elastoplastic translational or rotational spring with isotropic hardening)
Nonlinear elastic spring (nonlinear elastic translational or rotational spring with arbitrary force/displacement response moment/rotation dependency)
Nonlinear viscous damper (nonlinear damping with arbitrary force/velocity response moment/rotational velocity dependency)
General nonlinear spring (general nonlinear translational or rotational spring with arbitrary loading and unloading definitions)
Maxwell viscoelastic spring (Maxwell viscoelastic translational or rotational spring)
Inelastic tension or compressiononly spring (inelastic tension or compression only, translational or rotational spring)
SpringDamper (Discrete) Models in the ANSYS LSDYNA User's Guide.
NTEMP
:Number of temperatures for which data will be provided. Default = 1.
NPTS
:Number of data points to be specified for a given temperature. Default = 4 when
TBOPT
= MPDG
TBOPT
:Damage initiation definition:
Progressive damage evolution based on simple instant material stiffness reduction.
Progressive damage evolution based on continuum damage mechanics.
NTEMP
:Number of temperatures for which data will be provided. Default = 1.
NPTS
:Number of data points to be specified for a given temperature. Default = 4 when
TBOPT
= FCRT.
TBOPT
:Damage initiation definition:
Define failure criteria as the damage initiation criteria.
NTEMP
:Not used.
NPTS
:Not used.
TBOPT
:Not used.
NTEMP:
Not used.
NPTS:
Not used.
TBOPT:
Permittivity matrix options for PLANE223, SOLID226, and SOLID227:
Permittivity matrix at constant strain [ε^{S}] (used as supplied)
Permittivity matrix at constant stress [ε^{T}] (converted to [ε^{S}] form before use)
Anisotropic Electric Permittivity in the Material Reference.
NTEMP
:Number of temperatures for which data will be provided. Default = 1. Maximum = 40.
NPTS
:Number of data points to be specified for a given temperature.
TBOPT
:EDP material options.
Linear yield function.
Power law yield function.
Hyperbolic yield function.
Linear flow potential function.
Power law flow potential function.
Hyperbolic flow potential function.
Cap yield function.
Cap flow potential function.
See Extended DruckerPrager (EDP) in the Material Reference.
NTEMP:
Number of temperatures for which data will be provided.
NPTS:
Number of properties to be defined for the material option. This value is set
automatically according to the elasticity option (TBOPT
)
selected. If TBOPT
is not specified, default settings
become NPTS
= 2 and TBOPT
=
ISOT.
TBOPT:
Elasticity options:
Isotropic property (EX, NUXY) (default). Setting
NPTS
= 2 also selects this option automatically.
Orthotropic option with minor Poisson's ratio (EX, EY, EZ, GXY, GYZ, GXZ,
NUXY, NUYZ, NUXZ). NPTS
= 9. Setting
NPTS
= 9 selects this option automatically. All
nine parameters must be set, even for the 2D case.
Orthotropic option with major Poisson's ratio (EX, EY, EZ, GXY, GYZ, GXZ,
PRXY, PRYZ, PRXZ). NPTS
= 9. All nine parameters
must be set, even for the 2D case.
Anisotropic option in stiffness form (D11, D21, D31, D41, D51, D61, D22,
D32, D42, D52, D62, D33, D43, ..... D66). NPTS
=
21. Setting NPTS
= 21 selects this option
automatically.
Anisotropic option in compliance form (C11, C21, C31, C41, C51, C61, C22,
C32, C42, C52, C62, C33, C43, ..... C66). NPTS
=
21.
Userdefined linear elastic properties. For more information on the
user_tbelastic
subroutine, see the Guide to UserProgrammable Features in the Mechanical APDL Programmer's Reference.
See the TBFIELD command for more information about defining temperature and/or frequencydependent properties.
NTEMP
:Not used.
NPTS
:Not used.
TBOPT
:Equation of state (explicit dynamic elements only). No defaulta specified value is required.
JohnsonCook material model  for strain, strain rate, and temperature dependent impact/forming analyses.
Null material model  for allowing equation of state to be considered without computing deviatoric stresses.
ZerilliArmstrong material model  for metal forming processes in which the stress depends on strain, strain rate, and temperature.
Bamman material model  for metal forming processes with strain rate and
temperature dependent plasticity. Does not require an additional equation of
state (EOSOPT
is not used).
Steinberg material model  for modeling high strain rate effects in solid elements with failure.
NTEMP
:Not used.
NPTS
:Not used.
TBOPT
:Not used.
NTEMP
:Number of temperatures for which data will be provided.
NPTS
:Number of data points to be specified for a given temperature.
TBOPT
:Experimental data type:
Uniaxial tension experimental data.
Uniaxial compression experimental data.
Uniaxial experimental data (combined uniaxial tension and compression).
Equibiaxial experimental data.
Pure shear experimental data (also known as planar tension).
Simple shear experimental data.
Volumetric experimental data.
Shear modulus experimental data.
Bulk modulus experimental data.
Tensile modulus experimental data.
Poisson's ratio experimental data.
Experimental Data in the Material Reference.
Experimental Response Functions in the Mechanical APDL Theory Reference
Viscoelastic Material Model Material Reference.
See also the TBFIELD command documentation for information about defining fielddependent experimental data.
NTEMP
:Number of temperatures for which data will be provided. Default = 1. Maximum = 20.
NPTS
:Number of data points to be specified for a given temperature. Default = 1. Maximum = 100.
TBOPT
:Not used.
FLUID116 in the Element Reference.
NTEMP
:Number of temperatures for which data will be provided. Default = 1.
NPTS
:Number of data points to be specified for a given temperature. Default = 20 when
TBOPT
= 1. Default = 9 when
TBOPT
= 2.
TBOPT
:Material strength limit definition:
Define stressstrength limits.
Define strainstrength limits.
NTEMP:
Number of temperatures for which data will be provided. Default = 1.
NPTS:
Number of data points to be specified for a given temperature.
TBOPT:
Fluid material options:
Define material constants for a liquid material.
Define material constants for a gas material.
Define pressurevolume data for a fluid material.
Fluids in the Material Reference.
Fluid Material Models in the Mechanical APDL Theory Reference.
NTEMP
:Not used.
NPTS
:Not used.
TBOPT
:Foam material options for explicit dynamics elements. No defaulta specified value is required.
Rigid, closed cell, low density polyurethane foam material model.
Highly compressible urethane foam material model.
Energy absorbing foam material model.
Crushable foam material model.
NTEMP:
Number of temperatures for which data will be provided. Default = 1. No maximum limit.
NTEMP
is not used for the following situations:
Isotropic or orthotropic friction defined in terms of field data (TBFIELD command)
Userdefined friction (TBOPT
= USER)
NPTS:
Number of data points to be specified for userdefined friction
(TBOPT
= USER). Not used for
TBOPT
= ISO or TBOPT
=
ORTHO.
TBOPT:
Friction options:
Isotropic friction (one coefficient of friction, MU) (default). This option is valid for all 2D and 3D contact elements.
Orthotropic friction (two coefficients of friction, MU1 and MU2). This option is valid for the following 3D contact elements: CONTA173, CONTA174, CONTA175, CONTA176, and CONTA177.
Equivalent orthotropic friction (two coefficients of friction, MU1 and
MU2). This option differs from TBOPT
=ORTHO only in
the way the friction coefficients are interpolated when they are dependent
upon the following field variables: sliding distance and/or sliding velocity.
In this case, the total magnitude of the field variable is used to do the
interpolation.
User defined friction. This option is valid for all 2D and 3D contact elements.
Contact Friction in the Material Reference.
See also the TBFIELD command for more information about defining a coefficient of friction that is dependent on temperature, time, normal pressure, sliding distance, or sliding relative velocity.
NTEMP
:Number of temperatures for which data will be provided. Default = 1. The maximum
number of temperatures specified is such that NTEMP
*
NPTS
< 2000.
NPTS
:Number of data points to be specified for a given temperature. Default = 5 for
TBOPT
= PARA. Default = 1 for all other values of
TBOPT
.
TBOPT
:Gasket material options.
Gasket material general parameters.
Gasket material compression data.
Gasket linear unloading data.
Gasket nonlinear unloading data.
Transverse shear data.
Transverse shear and membrane stiffness data. (If selected, this option takes precedence over TSS.)
Gasket Materials in the Material Reference.
NTEMP
:Not used.
NPTS
:Not used.
TBOPT
:Not used.
Pressure Dependent Plasticity Models in the ANSYS LSDYNA User's Guide.
NTEMP
:Number of temperatures for which data will be provided. Default = 1. Maximum = 40.
NPTS
:Number of data points to be specified for a given temperature.
TBOPT
:GURSON material options.
Basic model without nucleation or coalescence (default).
Strain controlled nucleation.
Stress controlled nucleation.
Coalescence.
NTEMP
:Number of temperatures for which data will be provided. Default = 1. Maximum = 20.
NPTS
:Number of data points to be specified for a given temperature. Default = 1. Maximum = 100.
TBOPT
:Not used.
FLUID116 in the Element Reference.
NTEMP
:Number of temperatures for which data will be provided. Default = 1. Maximum = 40.
NPTS
:Not used.
TBOPT:
Hill plasticity option:
Use one set of Hill parameters (default).
Enter separate Hill parameters for plasticity and creep. This option is valid for material combinations of creep and Chaboche nonlinear kinematic hardening only.
Hill Yield Criterion in the Material Reference.
Also see Material Model Combinations.
NTEMP
:Number of temperatures for which data will be provided. Default = 1. The maximum
value of NTEMP
is such that
NTEMP
x NPTS
= 1000.
NPTS
:Number of data points to be specified for a given temperature, except for
TBOPT
= MOONEY, where NPTS
is
the number of parameters in the MooneyRivlin model (2 [default], 3, 5, or 9), and
TBOPT
= RESPONSE, where NPTS
is the number of terms in the volumetric strain energy polynomial.
TBOPT
:Hyperelastic material options.
ArrudaBoyce model. For NPTS
, default = 3 and
maximum = 3.
References:
ArrudaBoyce Hyperelasticity in the Material Reference.
ArrudaBoyce Hyperelastic Option in the Structural Analysis Guide.
BlatzKo model. For NPTS
, default = 1 and
maximum = 1.
References:
BlatzKo Foam Hyperelasticity in the Material Reference.
BlatzKo Hyperelastic Option in the Structural Analysis Guide.
Extended tube model. Five material constants
(NPTS
= 5) are required.
References:
Extended Tube Hyperelasticity in the Material Reference.
Extended Tube Model in the Mechanical APDL Theory Reference.
Hyperfoam (Ogden) model. For NPTS
, default = 1
and maximum is such that NTEMP
x
NPTS
x 3 = 1000.
References:
Ogden Compressible Foam Hyperelasticity in the Material Reference.
Ogden Compressible Foam Hyperelastic Option in the Structural Analysis Guide.
Gent model. For NPTS
, default = 3 and maximum =
3.
References:
MooneyRivlin model (default). You can choose a twoparameter
MooneyRivlin model with NPTS
= 2 (default), or a
three, five, or nineparameter model by setting
NPTS
equal to one of these values.
References:
MooneyRivlin Hyperelasticity in the Material Reference.
MooneyRivlin Hyperelastic Option in the Structural Analysis Guide.
NeoHookean model. For NPTS
, default = 2 and
maximum = 2.
References:
NeoHookean Hyperelasticity in the Material Reference.
NeoHookean Hyperelastic Option in the Structural Analysis Guide.
Ogden model. For NPTS
, default = 1 and maximum
is such that NTEMP
x
NPTS
x 3 = 1000.
References:
Polynomial form model. For NPTS
, default = 1
and maximum is such that NTEMP
x
NPTS
= 1000.
References:
Polynomial Form Hyperelasticity in the Material Reference.
Polynomial Form Hyperelastic Option in the Structural Analysis Guide.
Experimental response function model. For NPTS
,
default = 0 and maximum is such that NTEMP
x
NPTS
+ 2 = 1000.
References:
Response Function Hyperelasticity in the Material Reference.
Response Function Hyperelastic Option (TB,HYPER,,,,RESPONSE) in the Structural Analysis Guide.
Experimental Response Functions in the Mechanical APDL Theory Reference
Yeoh model. For NPTS
, default = 1 and maximum
is such that NTEMP
x
NPTS
x 2 = 1000.
References:
Userdefined hyperelastic model. See the ANSYS Guide to User Programmable Features for details.
References:
UserDefined Hyperelastic Material in the Material Reference.
UserDefined Hyperelastic Option in the Structural Analysis Guide.
NTEMP
:Number of temperatures for which data will be provided. Default = 1. No maximum
limit. NTEMP
is used only for userdefined contact
interaction (TBOPT
= USER).
NPTS
:Number of data points to be specified. NPTS
is used
only for userdefined contact interaction (TBOPT
=
USER).
TBOPT
:Contact interaction options.
The following options are valid only for general contact interactions specified via the GCDEF command:
Standard unilateral contact (default).
Rough, no sliding.
No separation (sliding permitted).
Bonded contact (no separation, no sliding).
No separation (always).
Bonded (always).
Bonded (initial contact).
The following option is valid for all 2D and 3D contact elements:
Userdefined contact interaction.
Contact Interaction in the Material Reference.
Defining Your Own Contact Interaction (USERINTER
) in the
Contact Technology Guide.
NTEMP:
Number of temperatures for which data will be provided. Default = 1.
NPTS:
Number of data points to be specified for a given temperature.
NPTS
is ignored if TBOPT
=
STIF or DAMP.
If Coulomb friction is specified, NPTS
is used only for
TBOPT
= MUS1, MUS4, and MUS6.
TBOPT:
Joint element material options.
Linear stiffness behavior:
Linear stiffness.
Nonlinear stiffness behavior:
Nonlinear stiffness behavior in all available components of relative motion for the joint element.
Nonlinear stiffness behavior in local UX direction only.
Nonlinear stiffness behavior in local UY direction only.
Nonlinear stiffness behavior in local UZ direction only.
Nonlinear stiffness behavior in local ROTX direction only.
Nonlinear stiffness behavior in local ROTY direction only.
Nonlinear stiffness behavior in local ROTZ direction only.
Linear damping behavior:
Linear damping.
Nonlinear damping behavior:
Nonlinear damping behavior in all available components of relative motion for the joint element.
Nonlinear damping behavior in local UX direction only.
Nonlinear damping behavior in local UY direction only.
Nonlinear damping behavior in local UZ direction only.
Nonlinear damping behavior in local ROTX direction only.
Nonlinear damping behavior in local ROTY direction only.
Nonlinear damping behavior in local ROTZ direction only.
Friction Behavior:
The values can be specified using either TBDATA
(NPTS
= 0) or TBPT
(NPTS
is nonzero).
Coulomb friction coefficient (stiction) in local UX direction only.
Coulomb friction coefficient (stiction) in local ROTX direction only.
Coulomb friction coefficient (stiction) in local ROTZ direction only.
Use TBDATA to specify μ_{s}, μ_{d}, and c for the exponential law.
Exponential law for friction in local UX direction only.
Exponential law for friction in local ROTX direction only.
Exponential law for friction in local ROTZ direction only.
Elastic slip:
Elastic slip in local UX direction only.
Elastic slip in local ROTX direction only.
Elastic slip in local ROTZ direction only.
Critical force in local UX direction only.
Critical moment in local ROTX direction only.
Critical moment in local ROTZ direction only.
Stickstiffness:
Stickstiffness in local UX direction only.
Stickstiffness in local ROTX direction only.
Stickstiffness in local ROTZ direction only.
Interference fit force/moment:
Interference fit force in local UX direction only.
Interference fit moment in local ROTX direction only.
Interference fit moment in local ROTZ direction only.
MPC184 Joint in the Material Reference.
NTEMP
:Not used.
NPTS
:Not used.
TBOPT
:Base material parameters.
Base material tension cutoff.
Residual strength coupling.
Joint parameters.
Joint tension cutoff.
Joint orientation.
NTEMP
:Not used.
NPTS
:Not used.
TBOPT
:MohrCoulomb material parameters.
Tension cutoff.
Residual strength coupling.
NTEMP
:Not used.
NPTS
:Not used.
TBOPT
:Migration model options.
Atomic (or ion) flux (default).
Vacancy flux.
Migration Model in the Material Reference.
ElectricDiffusion Analysis, ThermalDiffusion Analysis, and StructuralDiffusion Analysis in the CoupledField Analysis Guide.
ElectricDiffusion Coupling, ThermalDiffusion Coupling, and StructuralDiffusion Coupling in the Mechanical APDL Theory Reference.
NTEMP
:Number of temperatures for which data will be provided. Default = 6. Maximum = 6.
NPTS
:(Not used for explicit dynamic elements.)
TBOPT
:MooneyRivlin material option, applicable to explicit dynamic elements PLANE162, SHELL163, SOLID164, and SOLID168.
Direct input of hyperelastic material constants (default).
Reserved for future use.
Material constants to be calculated by the LSDYNA program from experimental data. This option is only valid for explicit dynamic elements.
NTEMP
:The number of temperatures for which data will be provided. Default = 1. Maximum
is such that NTEMP
x NPTS
=
1000.
NPTS
:Number of material constants (six total).
TBOPT
:Not used.
Microplane in the Material Reference.
NTEMP
:Number of temperatures for which data will be provided. Default = 1. Maximum = 20.
NPTS
:Number of data points to be specified for a given temperature. Default = 4. Maximum = 4.
TBOPT
:Isotropic hardening options.
Voce hardening law (default).
Power hardening law.
NTEMP:
Not used.
NPTS:
Not used.
TBOPT:
Equivalent fluid model options:
JohnsonChampouxAllard model
DelaneyBazley model
Miki model
Complex impedance and propagating constant model
Complex density and velocity model
Transfer admittance matrix model
Transfer admittance matrix model of square grid structure
Transfer admittance matrix model of hexagonal grid structure
Defining Acoustic Material Properties in the Acoustic Analysis Guide.
Equivalent Fluid Model of Perforated Media in the Material Reference .
Equivalent Fluid of Perforated Materials in the Mechanical APDL Theory Reference
See the TBFIELD command for more information about defining temperature and/or frequencydependent properties.
NTEMP
:Not used.
NPTS
:Not used.
TBOPT
:Piezoelectric matrix options.
Piezoelectric stress matrix [e] (used as supplied)
Piezoelectric strain matrix [d] (converted to [e] form before use)
Piezoelectricity in the Material Reference.
NTEMP:
Not used.
NPTS:
Not used.
TBOPT:
Plasticity option:
Multilinear kinematic hardening plasticity.
The number of points (TBPT commands issued) is limited to 100 for this option.
NTEMP
:Not used.
NPTS
:Not used.
TBOPT
:Plasticity options for explicit dynamics elements. No defaulta specified value is required.
Isotropic/kinematic hardening model.
Strain rate dependent plasticity model used for metal and plastic forming analyses.
Anisotropic plasticity model (Barlat and Lian).
Strain rate dependent plasticity model used for superplastic forming analyses.
Strain rate dependent isotropic plasticity model used for metal and plastic forming analyses.
Anisotropic plasticity model (Barlat, Lege, and Brem) used for forming processes.
Fully iterative anisotropic plasticity model for explicit shell elements only.
Piecewise linear plasticity model for explicit elements only.
Elasticplastic hydrodynamic model for explicit elements only.
Transversely anisotropic FLD (flow limit diagram) model for explicit elements only.
Modified piecewise linear plasticity model for explicit shell elements only.
Elastic viscoplastic thermal model for explicit solid and shell elements only.
Nonlinear Inelastic Models in the ANSYS LSDYNA User's Guide.
Pressure Dependent Plasticity Models in the ANSYS LSDYNA User's Guide.
NTEMP
:Not used.
NPTS
:Not used.
TBOPT
:Porous elasticity model..
NTEMP
:The number of temperatures. Default = 1. The maximum must be a value such that
(NTEMP
x NPTS
) <=
1000.
NPTS
:The number of material constants. Default = 4. The maximum must be a value such
that (NTEMP
x NPTS
) <=
1000.
TBOPT
: Porous media options:
Permeability
Biot coefficient
Solid property
Fluid property
Degreeofsaturation table
Relativepermeability table
Gravity magnitude
Porous Media Material Properties in the Mechanical APDL Material Reference.
Porous Media Flow in the Mechanical APDL Theory Reference.
StructuralPoreFluidDiffusionThermal Analysis in the Mechanical APDL CoupledField Analysis Guide.
Also see VM260.
NTEMP:
Number of temperatures for which data will be provided. Default = 1. Maximum = 100.
Unused for TBOPT
= EXPERIMENTAL.
NPTS:
Defines the number of Prony series pairs for TBOPT
=
SHEAR or TBOPT
= BULK. Default = 1. Maximum = 100.
The number of temperatures and Prony pairs specified should be such that
NTEMP
* 2 * NPTS
<
1000.
Unused for TBOPT
= INTEGRATION and
TBOPT
= EXPERIMENTAL.
TBOPT:
Defines the behavior for viscoelasticity.
Shear Prony series.
Bulk Prony series.
Stress update algorithm.
Complex modulus from experimental data.
Viscoelasticity in the Material Reference.
NTEMP:
Not used.
NPTS:
Not used.
TBOPT:
Piezoresistive matrix options
Piezoresistive stress matrix (used as supplied)
Piezoresistive strain matrix (used as supplied)
Piezoresistivity in the Material Reference.
Piezoresistive Analysis in the CoupledField Analysis Guide.
NTEMP
:The number of temperatures for which data will be provided. Default is 1. Maximum
is such that NTEMP
x NPTS
=
1000.
NPTS
:The number of data points to be specified for a given temperature. Default = 2.
Maximum is such that NTEMP
x
NPTS
= 1000.
TBOPT
:Ratedependent viscoplasticity options.
Perzyna option (default).
Peirce option.
Exponential viscohardening option.
Anand option.
RateDependent Plasticity (Viscoplasticity) in the Material Reference.
Viscoplasticity in the Structural Analysis Guide.
RateDependent Plasticity in the Mechanical APDL Theory Reference.
See also Material Model Combinations.
NTEMP:
Number of temperatures for which data will be provided. Default = 1.
NPTS:
Number of properties to be defined for the material option. Default = 1 for each
material damping option (TBOPT
) selected.
TBOPT:
Material damping options:
Structural damping coefficient (default).
Rayleigh mass proportional material damping.
Rayleigh stiffness proportional material damping.
NTEMP:
Allows one temperature for which data will be provided.
NPTS:
Number of material constants to be entered as determined by the shift function
specified by TBOPT
.
for TBOPT
= 1 or WLF
for TBOPT
= 2 or TN
n
_{
f
}
for TBOPT
= 3 or FICT, where
n
_{
f
}
is the number of partial fictive temperatures
TBOPT:
Defines the shift function
WilliamsLandelFerry shift function
ToolNarayanaswamy shift function
ToolNarayanaswamy with fictive temperature shift function
(or USER) Userdefined shift function.
Viscoelasticity in the Material Reference.
NTEMP
:Number of temperatures for which data will be provided. Default = 1.
NPTS
:Number of data points to be specified for a given temperature. Default = 6 if
TBOPT
= SUPE, or 7 otherwise.
TBOPT
:Shape memory model option:
SUPE  Superelasticity option (default).
MEFF  Memoryeffect option.
Because the material tangent stiffness matrix is generally unsymmetric, convergence problems typically occur when
TBOPT
= MEFF and the (default) full NewtonRaphson option (NROPT,FULL) is in effect; therefore, use the unsymmetric NewtonRaphson option (NROPT,UNSYM) whenTBOPT
= MEFF.
NTEMP
:Not used.
NPTS
:Not used.
TBOPT
:Modified Camclay material model.
When Lab
= STATE is applied to userdefined materials, the
state variable specifications affect either the
UserMat
(userdefined
material) or
UserMatTh
(userdefined thermal material) subroutine, as
appropriate. The subroutine in use depends on the element type used when
Lab
= USER is specified.
NTEMP
:Not used.
NPTS
:Number of state variables.
TBOPT
:Not used.
Using State Variables with UserDefined Materials in the Material Reference.
NTEMP
:Number of temperatures for which data will be provided. The maximum value of NTEMP is such that NTEMP x NPTS = 1000
NPTS
:Number of data points to be specified for a given temperature. The maximum value of NPTS is such that NPTS x NTEMP = 1000.
TBOPT
:Swelling model options:
Linear swelling function.
Exponential swelling function.
Userdefined swelling function. Define the swelling function via
subroutine
usersw
(described in the Programmer's Reference). Define temperaturedependent constants
via the TBTEMP and TBDATA commands. For
solutiondependent variables, define the number of variables via the
TB,STATE command.
Swelling in the Material Reference.
Swelling in the Structural Analysis Guide.
NTEMP
:Not used.
NPTS
:Not used.
TBOPT
:Thermal properties:
Thermal conductivity.
Specific heat.
Thermal Properties in the Material Reference.
NTEMP:
Number of temperatures for which data will be provided. Default = 1. Maximum = 10.
NPTS:
Number of data points to be specified for a given temperature. Default = 20. Maximum = 20.
TBOPT:
Defines stressstrain relationship for cast iron plasticity.
Defines stressstrain relation in tension
Defines stressstrain relation in compression.
Cast Iron in the Material Reference.
When Lab
= USER, the TB command activates
either the
UserMat
(userdefined material) or the
UserMatTh
(userdefined thermal material) subroutine
automatically. The subroutine activated depends on the element type used.
NTEMP
:Number of temperatures for which data will be provided. Default = 1.
NPTS
:Number of data points to be specified for a given temperature. Default = 48.
TBOPT:
Userdefined material model (
UserMat
) or thermal
material model (
UserMatTh
) options:
Nonlinear iterations are applied (default).
Nonlinear iterations are not applied. This option is ignored if there is any other nonlinearity involved, such as contact, geometric nonlinearity, etc.
This option indicates a UserMat material model to be used with mixed uP element formulation for material exhibiting incompressible or nearly incompressible behavior.
UserDefined Material Model (UserMat) in the Material Reference.
Subroutine UserMat (Creating Your Own Material Model) in the Programmer's Reference.
Subroutine UserMatTh (Creating Your Own Thermal Material Model) in the Programmer's Reference.
NTEMP:
Number of temperatures for which data will be provided.
NPTS:
Number of data points to be specified for the wear option. This value is set
automatically based on the selected wear option (TBOPT
). If
TBOPT
is not specified, the default becomes
NPTS
= 5 and TBOPT
=
ARCD.
TBOPT:
Wear model options:
Archard wear model (default).
Userdefined wear model.
Contact Surface Wear in the Material Reference.
See also the TBFIELD command for more information on defining temperature and/or timedependent properties.
TB activates a data table to be used with subsequent TBDATA or TBPT commands. The table space is initialized to zero values. Data from this table are used for certain nonlinear material descriptions as well as for special input for some elements.
For a list of elements supporting each material model (Lab
value), see Material Model Element Support in the Material Reference.
For a description of data table input required for explicit dynamic materials, see Material Models in the ANSYS LSDYNA User's Guide.
For information about linear material property input, see the MP command.
This command is also valid in SOLUTION.
Command Option Lab  Available Products 
AFDM  –  –  Enterprise  Ent PP  Ent Solver  – 
AHYPER  –  –  Enterprise  Ent PP  Ent Solver  – 
ANEL  Pro  Premium  Enterprise  Ent PP  Ent Solver  – 
BB  –  –  Enterprise  Ent PP  Ent Solver  – 
BH  –  –  Enterprise  Ent PP  Ent Solver  – 
BISO  –  Premium  Enterprise  Ent PP  Ent Solver  – 
BKIN  –  Premium  Enterprise  Ent PP  Ent Solver  – 
BB  –  –  Enterprise  Ent PP  Ent Solver  – 
CAST  –  –  Enterprise  Ent PP  Ent Solver  – 
CDM  –  –  Enterprise  Ent PP  Ent Solver  – 
CGCR  –  –  Enterprise  Ent PP  Ent Solver  – 
CHABOCHE  –  Premium  Enterprise  Ent PP  Ent Solver  – 
COMP  –  –  Enterprise  Ent PP  Ent Solver  – 
CONCR  –  Premium  Enterprise  Ent PP  Ent Solver  – 
CREEP  –  –  Enterprise  Ent PP  Ent Solver  – 
CTE  Pro  Premium  Enterprise  Ent PP  Ent Solver  – 
CZM  –  –  Enterprise  Ent PP  Ent Solver  – 
CNDE  –  –  Enterprise  Ent PP  Ent Solver  – 
CNDM  –  –  Enterprise  Ent PP  Ent Solver  – 
DISCRETE  –  –  Enterprise  Ent PP  Ent Solver  – 
DMGE  –  –  Enterprise  Ent PP  Ent Solver  – 
DMGI  –  –  Enterprise  Ent PP  Ent Solver  – 
DP  –  –  Enterprise  Ent PP  Ent Solver  – 
DPER  –  –  Enterprise  Ent PP  Ent Solver  – 
EDP  –  –  Enterprise  Ent PP  Ent Solver  – 
ELASTIC  Pro  Premium  Enterprise  Ent PP  Ent Solver  – 
ELASTIC (TBOPT = USER)  –  –  Enterprise  Ent PP  Ent Solver  – 
EOS  –  –  Enterprise  Ent PP  Ent Solver  – 
EVISC  –  –  Enterprise  Ent PP  Ent Solver  – 
EXPE  –  –  Enterprise  Ent PP  Ent Solver  – 
FCON  –  –  Enterprise  Ent PP  Ent Solver  – 
FCLI  –  Premium  Enterprise  Ent PP  Ent Solver  – 
FLUID  –  –  Enterprise  Ent PP  Ent Solver  – 
FOAM  –  –  Enterprise  Ent PP  Ent Solver  – 
FRIC  –  –  Enterprise  Ent PP  Ent Solver  – 
GASKET  –  –  Enterprise  Ent PP  Ent Solver  – 
GCAP  –  –  Enterprise  Ent PP  Ent Solver  – 
HFLM  Pro  Premium  Enterprise  Ent PP  Ent Solver  – 
HILL  –  –  Enterprise  Ent PP  Ent Solver  – 
HONEY  –  –  Enterprise  Ent PP  Ent Solver  – 
HYPER  –  Premium  Enterprise  Ent PP  Ent Solver  – 
HYPER (TBOPT = USER)  –  –  Enterprise  Ent PP  Ent Solver  – 
INTER  Pro  Premium  Enterprise  Ent PP  Ent Solver  – 
INTER (TBOPT = USER)  –  –  Enterprise  Ent PP  Ent Solver  – 
JOIN  –  Premium  Enterprise  Ent PP  Ent Solver  – 
JOIN (TBOPT = STIF)  Pro  Premium  Enterprise  Ent PP  Ent Solver  – 
JROCK  –  –  Enterprise  Ent PP  Ent Solver  – 
MC  –  –  Enterprise  Ent PP  Ent Solver  – 
MOONEY  –  Premium  Enterprise  Ent PP  Ent Solver  – 
MPLANE  –  Premium  Enterprise  Ent PP  Ent Solver  – 
NLISO  –  Premium  Enterprise  Ent PP  Ent Solver  – 
PELAS  –  –  Enterprise  Ent PP  Ent Solver  – 
PERF  –  –  Enterprise  Ent PP  Ent Solver  – 
PIEZ  –  –  Enterprise  Ent PP  Ent Solver  – 
PLASTIC  –  Premium  Enterprise  Ent PP  Ent Solver  – 
PLAW  –  –  Enterprise  Ent PP  Ent Solver  – 
PRONY  –  –  Enterprise  Ent PP  Ent Solver  – 
PZRS  –  –  Enterprise  Ent PP  Ent Solver  – 
RATE  –  –  Enterprise  Ent PP  Ent Solver  – 
SDAMP  –  Premium  Enterprise  Ent PP  Ent Solver  – 
SHIFT  –  –  Enterprise  Ent PP  Ent Solver  – 
SMA  –  –  Enterprise  Ent PP  Ent Solver  – 
SOIL  –  –  Enterprise  Ent PP  Ent Solver  – 
STATE  –  –  Enterprise  Ent PP  Ent Solver  – 
SWELL  –  –  Enterprise  Ent PP  Ent Solver  – 
UNIAXIAL  –  –  Enterprise  Ent PP  Ent Solver  – 
USER  –  –  Enterprise  Ent PP  Ent Solver  – 
WEAR  –  –  Enterprise  Ent PP  Ent Solver  – 