MP ME ST PR PRN <> <> <> EM EH DY PP <> EME MFS

For a list of elements supporting each material model (*Lab* value), see "Element Support for Material Models" in the *Material Reference*.

*Lab*Material model data table type:

**AHYPER**— **ANEL**— **ANISO**— **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**— Fracture criterion for crack growth simulation (

**CGROW**).**CHABOCHE**— Chaboche nonlinear kinematic hardening using von Mises or Hill plasticity.

**CNDE**— **CNDM**— **COMP**— **CONCR**— Concrete element data.

**CREEP**— Creep. Pure creep, creep with isotropic hardening plasticity, or creep with kinematic hardening plasticity using both von Mises or Hill potentials.

**CZM**— **DISCRETE**— Explicit spring-damper (discrete).

**DMGE**— **DMGI**— **DP**— **DPER**— **EDP**— Extended Drucker-Prager (for granular materials such as rock, concrete, soil, ceramics and other pressure-dependent materials).

**ELASTIC**— Elasticity. For full harmonic analyses, properties can be defined as frequency- or temperature-dependent (

**TBFIELD**).**EOS**— Equation of state (explicit dynamic analysis).

**EVISC**— Viscoelastic element data (explicit dynamic analysis).

**EXPE**— **FCON**— **FCLI**— Material strength limits for calculating failure criteria.

**FLUID**— **FOAM**— Foam (explicit dynamic analysis).

**FRIC**— Coefficient of friction based on Coulomb's Law or user-defined friction.

**GASKET**— **GCAP**— Geological cap (explicit dynamic analysis).

**GURSON**— Gurson pressure-dependent plasticity for porous metals.

**HFFDLD**— **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 (Arruda-Boyce, Blatz-Ko, Extended Tube, Gent, Mooney-Rivlin [default], Neo-Hookean, Ogden, Ogden Foam, Polynomial Form, Response Function, Yeoh, and user-defined).

**JOIN**— Joint (linear and nonlinear elastic stiffness, linear and nonlinear damping, and frictional behavior).

**KINH**— Multilinear kinematic hardening using von Mises or Hill plasticity.

**LSEM**— **MELAS**— **MISO**— Multilinear isotropic hardening using von Mises or Hill plasticity.

**MKIN**— Multilinear kinematic hardening using von Mises or Hill plasticity.

**MOONEY**— Mooney-Rivlin hyperelasticity (explicit dynamic analysis).

**MPLANE**— **MUR**— **NLISO**— Voce isotropic hardening law (or power law) for modeling nonlinear isotropic hardening using von Mises or Hill plasticity.

**PIEZ**— **PLASTIC**— Nonlinear plasticity with stress-vs.-plastic strain data.

**PLAW**— Plasticity laws (explicit dynamic analysis).

**PM**— **PRONY**— Prony series constants for viscoelastic materials.

**PZRS**— **RATE**— Rate-dependent plasticity (viscoplasticity) when combined with the BISO, MISO, NLISO or PLASTIC material options, or rate-dependent anisotropic plasticity (anisotropic viscoplasticity) when combined with the HILL and BISO, MISO, NLISO or PLASTIC material options.

The exponential visco-hardening 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 structural damping coefficient. For full harmonic analyses, damping coefficients can be defined as frequency- or temperature-dependent properties (

**TBFIELD**). SDAMP specifies damping in terms of the loss factor, which is equal to 2x the damping ratio.For the relationship between SDAMP,

**DMPRAT**and**MP**,BETD, see "Notes".When specifying frequency-dependent damping, specify the material property via

**TB**,ELAS.**SHIFT**— Shift function for viscoelastic materials.

**SMA**— Shape memory alloy for simulating hysteresis superelastic behavior with no performance degradation. Plane stress is not supported.

**STATE**— User-defined state variables. Valid with

**TB**,USER and used with the UserMat subroutine. Also valid with**TB**,CREEP (when*TBOPT*= 100) and used with the UserCreep subroutine.**SWELL**— Swelling strain function.

**UNIAXIAL**— Uniaxial stress-strain relation associated with the Cast iron material model.

**USER**— User-defined material model (general-purpose except for incompressible material models).

*MAT*Material reference number. The default value is 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 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 is a listing of all valid **TB** command
labels (*Lab* values). For each material
type, the data table includes requirements for the *NTEMP*, *NPTS*, and *TBOPT* options, along with links to more detailed documentation if needed.

- "Kinematic Hardening Tables"
- "Isotropic Hardening Tables"
- "Anisotropic Plasticity Tables "
- "Nonmetal and Other Plasticity Tables"
- "Elasticity Tables "
- "Rate-Dependent Plasticity Tables"
- "Hyperelasticity Tables "
- "Viscoelasticity Tables "
- "Multiphysics Tables"
- "Porous Media Tables"
- "ANSYS LS-DYNA Tables"
- "Special Material Tables"
- "User Tables"

*NTEMP*:Number of temperatures for which data will be provided. Default = 6. Maximum = 6.

*NPTS*:Not used.

*TBOPT*:Stress-strain options (not used in an explicit dynamics analysis).

**0 --**No stress relaxation with temperature increase (this is not recommended for nonisothermal problems).

**1 --**Rice's hardening rule, which takes into account stress relaxation with increasing temperature. This value is the default.

**References:**Bilinear Kinematic Hardening in the

*Material Reference*.Plastic Material Options in the

*Structural Analysis Guide*.Nonlinear Inelastic Models in the

*ANSYS LS-DYNA User's Guide*.

*NTEMP*:Number of temperatures for which data will be provided. Default = 1. The maximum value of

*NTEMP*is such that*NTEMP*x (1 + 2*NPTS*) = 1000.*NPTS*:Number of kinematic models to be superposed. Default = 1. Maximum value of

*NPTS*is such that*NTEMP*x (1 + 2*NPTS*) = 1000.*TBOPT*:Not used.

**References:**

This material is the same as MKIN with *TBOPT* = 2, but with fewer
restrictions on the number of points per curve and the number of temperatures.

*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. Default = 20, Maximum = 20

*TBOPT*:Use 0 or leave blank to define stress -vs- total strain curve.

Use 4 or enter “PLASTIC” to define stress -vs- plastic strain curve. This option supports only elements LINK180, SHELL181, PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, BEAM188, BEAM189, SOLSH190, SHELL208, SHELL209, REINF264, REINF265, SOLID272, SOLID273, SOLID285, SHELL281, PIPE288, PIPE289, and ELBOW290, .

**References:**

*NTEMP*:Number of temperatures for which data will be provided. Default = 5. Maximum = 5.

*NPTS*:Not used.

*TBOPT*:Stress-strain options.

**0 --**No stress relaxation with temperature increase (this is not recommended for nonisothermal problems); also produces thermal ratcheting. This value is the default.

**1 --**Recalculate total plastic strain using new weight factors of the subvolume.

**2 --**Scale layer plastic strains to keep total plastic strain constant; agrees with Rice's model (

**TB**, BKIN with*TBOPT*= 1). Produces stable stress-strain cycles.

**References:**

*NTEMP*:Number of temperatures for which data will be provided. Default = 6. Maximum = 6.

*NPTS*:Not used.

*TBOPT*:Not used.

**References:**Bilinear Isotropic Hardening in the

*Material Reference*.Plastic Material Options in the

*Structural Analysis Guide*.Nonlinear Inelastic Models in the

*ANSYS LS-DYNA User's Guide*.

*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 = 20. Maximum = 100.

*TBOPT*:Not used.

**References:**

*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 --**Voce hardening law. This value is the default.

**POWER --**Power hardening law.

**References:**

*NTEMP:*The number of temperature points (default = 1). You can specify up to 20.

*NPTS:*The number of stress versus plastic strain data points (default = 20). You can specify up to 100.

*TBOPT:*Type of plastic hardening:

**MISO --**Multilinear isotropic hardening plasticity.

**KINH --**Multilinear kinematic hardening plasticity.

**References:**Plasticity in the

*Structural Analysis Guide*.Multilinear Kinematic Hardening and Multilinear Isotropic Hardening in the

*Material Reference*.

*NTEMP*:Not used.

*NPTS*:Not used.

*TBOPT*:Not used.

**References:**Anisotropic in the

*Material Reference*.

*NTEMP*:Number of temperatures for which data will be provided. Default = 1. Maximum = 40.

*NPTS*:Not used.

*TBOPT*:Not used.

**References:**Hill's Anisotropy in the

*Material Reference*.Plastic Material Options in the

*Structural Analysis Guide*.Also see Material Model Combinations.

*NTEMP:*Number of temperatures for which data will be provided. Default = 1; Max = 10.

*NPTS:*Not used.

*TBOPT:*Defines hardening type.

**ISOTROPIC --**Specifies cast iron plasticity with isotropic hardening.

**References:**

*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.

**References:**SOLID65 in the

*Element Reference*.

*NTEMP*:Not used.

*NPTS*:Not used.

*TBOPT*:Not used.

**References:**Drucker-Prager 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.

*TBOPT*:EDP material options.

**LYFUN --**LInear yield function.

**PYFUN --**Power law yield function.

**HYFUN --**Hyperbolic yield function.

**LFPOT --**Linear flow potential function.

**PFPOT --**Power law flow potential function.

**HFPOT --**Hyperbolic flow potential function.

**CYFUN --**Cap yield function.

**CFPOT --**Cap flow potential function.

**References:**See Extended Drucker-Prager in the

*Material Reference*.Also see Plastic Material Options 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*:GURSON material options.

**BASE --**Basic model without nucleation or coalescence. This value is the default.

**SNNU --**Strain controlled nucleation.

**SSNU --**Stress controlled nucleation.

**COAL --**Coalescence

**References:**See Gurson's Model in the

*Material Reference*.Also see Plastic Material Models and Gurson-Chaboche 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.

*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:****STIF --**Linear stiffness.

**Nonlinear stiffness behavior:****JNSA --**Nonlinear stiffness behavior in all available components of relative motion for the joint element.

**JNS1 --**Nonlinear stiffness behavior in local UX direction only.

**JNS2 --**Nonlinear stiffness behavior in local UY direction only.

**JNS3 --**Nonlinear stiffness behavior in local UZ direction only.

**JNS4 --**Nonlinear stiffness behavior in local ROTX direction only.

**JNS5 --**Nonlinear stiffness behavior in local ROTY direction only.

**JNS6 --**Nonlinear stiffness behavior in local ROTZ direction only.

**Linear damping behavior:****DAMP --**Linear damping.

**Nonlinear damping behavior:****JNDA --**Nonlinear damping behavior in all available components of relative motion for the joint element.

**JND1 --**Nonlinear damping behavior in local UX direction only.

**JND2 --**Nonlinear damping behavior in local UY direction only.

**JND3 --**Nonlinear damping behavior in local UZ direction only.

**JND4 --**Nonlinear damping behavior in local ROTX direction only.

**JND5 --**Nonlinear damping behavior in local ROTY direction only.

**JND6 --**Nonlinear damping behavior in local ROTZ direction only.

**Friction Behavior:****Coulomb friction coefficient -**The values can be specified using either

**TBDATA**(*NPTS*= 0) or**TBPT**(*NPTS*is nonzero).**MUS1 --**Coulomb friction coefficient (stiction) in local UX direction only.

**MUS4 --**Coulomb friction coefficient (stiction) in local ROTX direction only.

**MUS6 --**Coulomb friction coefficient (stiction) in local ROTZ direction only.

**Coulomb friction coefficient - Exponential Law -**Use

**TBDATA**to specify μ_{s}, μ_{d}, and c for the exponential law.**EXP1 --**Exponential law for friction in local UX direction only.

**EXP4 --**Exponential law for friction in local ROTX direction only.

**EXP6 --**Exponential law for friction in local ROTZ direction only.

**Elastic slip:****SL1 --**Elastic slip in local UX direction only.

**SL4 --**Elastic slip in local ROTX direction only.

**SL6 --**Elastic slip in local ROTZ direction only.

**TMX1 --**Critical force in local UX direction only.

**TMX4 --**Critical moment in local ROTX direction only.

**TMX6 --**Critical moment in local ROTZ direction only.

**Stick-stiffness:****SK1 --**Stick-stiffness in local UX direction only.

**SK4 --**Stick-stiffness in local ROTX direction only.

**SK6 --**Stick-stiffness in local ROTZ direction only.

**Interference fit force/moment:****FI1 --**Interference fit force in local UX direction only.

**FI4 --**Interference fit moment in local ROTX direction only.

**FI6 --**Interference fit moment in local ROTZ direction only.

**References:**

*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 = 7.

*TBOPT*:Shape memory model option:

1 or SUPE -- Superelasticity option.

2 or MEFF -- Memory effect option.

**Reference:**Shape Memory Alloy (SMA) Material Model in the

*Material Reference*.

*NTEMP:*Number of temperatures for which data will be provided. Default = 1; Max = 10.

*NPTS:*Number of data points to be specified for a given temperature. Default = 20; Max = 20.

*TBOPT:*Defines stress-strain relationship for cast iron plasticity.

**TENSION --**Defines stress-strain relation in tension

**COMPRESSION --**Defines stress-strain relation in compression.

**References:**

*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.

**0 --**Elasticity matrix used as supplied (input in stiffness form).

**1 --**Elasticity matrix inverted before use (input in flexibility form). This option is not valid for explicit dynamic elements.

**References:**Anisotropic Elastic Material Model in the

*Material Reference*.

*NTEMP:*Not used.

*NPTS:*Number of properties to be defined for the material option. This value is set automatically based on the elasticity option (

*TBOPT*) selected. If*TBOPT*is not specified, it is set to ISOT by default and*NPTS*is set to 2.*TBOPT:*Elasticity options:

**ISOT --**Isotropic property (EX, NUXY). This is the default value.

*NPTS*= 2. Setting*NPTS*= 2 selects this option automatically.**OELN --**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 2-D case.**OELM --**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 2-D case.**AELS --**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.**AELF --**Anisotropic option in compliance form (C11, C21, C31, C41, C51, C61, C22, C32, C42, C52, C62, C33, C43, ..... C66).

*NPTS*= 21.**USER --**User-defined linear elastic properties. For more information, see the documentation for the user_tbelastic subroutine in the

*Guide to ANSYS User Programmable Features*.

**References:**See the

**TBFIELD**command for more information about defining temperature and/or frequency-dependent properties.

*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 = 20. Maximum = 100.

*TBOPT*:Not used.

**References:**

*NTEMP:*Not used.

*NPTS:*Number of properties to be defined for the material option.

**1 --**Structural damping coefficient. This is the default.

*TBOPT:*Not Used.

**References:**See the

**TBFIELD**command for more information about defining temperature and/or frequency dependent properties.

*NTEMP*:Number of temperatures for which data will be provided. Default = 1. Maximum value of

*NTEMP*is such that*NTEMP*x*NPTS*= 1000 for implicit creep and 250 for explicit creep.*NPTS*:Number of data points to be specified for a given temperature. Default = 12 for implicit creep and 72 for explicit creep. Maximum value of

*NPTS*is such that*NTEMP*x*NPTS*= 1000 for implicit creep and 250 for explicit creep.*TBOPT*:Creep model options.

**0 --**(or Blank) Explicit creep option. Creep model is defined by constants C

_{6}, C_{12}, and C_{66}, through**TBDATA**. See Primary Explicit Creep Equation for C6 = 0 through Irradiation Induced Explicit Creep Equation for C66 = 5 for the associated equations. (Applicable to SOLID62 and 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 ANSYS User Programmable Features*for more information.**1 through 13 --**Implicit creep option. See Table 3.2: "Implicit Creep Equations" for a list of available equations. Use

**TBTEMP**and**TBDATA**to define temperature-dependent 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).**100 --**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 ANSYS User Programmable Features*for more information. Use**TBTEMP**and**TBDATA**to define temperature-dependent constants. For implicit creep, use with**TB**,STATE for defining the number of state variables.

**References:**Creep Equations in the

*Material Reference*.Creep in the

*Structural Analysis Guide*.See also Material Model Combinations.

*NTEMP*:The number of temperatures for which data will be provided. The default is 1. The maximum

*NTEMP*value is such that*NTEMP*x*NPTS*= 1000.*NPTS*:Number of material constants (six total).

*TBOPT*:Not used.

**References:**

*NTEMP*:The number of temperatures for which data will be provided. The default is 1. The maximum

*NTEMP*value is such that*NTEMP*x*NPTS*= 1000.*NPTS*:The number of data points to be specified for a given temperature. The default is 2. The maximum

*NPTS*value is such that*NTEMP*x*NPTS*= 1000.*TBOPT*:Rate-dependent viscoplasticity options.

**PERZYNA --**Perzyna option (default).

**PEIRCE --**Peirce option.

**EVH --**Exponential visco-hardening option.

**ANAND --**Anand option.

**References:**Rate-Dependent Plastic (Viscoplastic) Material Models in the

*Material Reference*.Viscoplasticity in the

*Structural Analysis Guide*.Rate-Dependent Plasticity in the

*Mechanical APDL Theory Reference*.See also Material Model Combinations.

*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 --**Linear swelling function.

**EXPT --**Exponential swelling function.

**USER --**User-defined swelling function. Define the swelling function via subroutine usersw (described in

*Guide to ANSYS User Programmable Features*). Define temperature-dependent constants via the**TBTEMP**and**TBDATA**commands. For solution-dependent variables, define the number of variables via the**TB**,STATE command.

**References:**Swelling Model in the

*Material Reference*.Swelling 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*:Anisotropic hyperelastic material options.

**POLY --**Anisotropic potential.

**EXPO --**Exponential strain energy potential.

**AVEC --**Define the A vector.

**BVEC --**Define the B vector.

**PVOL --**Volumetric potential.

**References:**Anisotropic Hyperelasticity in the

*Material Reference*.Anisotropic Hyperelasticity in the

*Mechanical APDL Theory 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 material constants. If

*TBOPT*= ISO, then*NPTS*= 7. If*TBOPT*= 1, then*NPTS*= 1.*TBOPT*:Isochoric or volumetric strain-energy function:

**ISO --**Define material constants for isochoric strain energy.

**PVOL --**Define material constants for volumetric strain energy.

**References:**Bergstrom-Boyce in the

*Mechanical APDL Theory Reference*.Bergstrom-Boyce Material in the

*Material Reference*.Bergstrom-Boyce Hyperviscoelastic Material Model in the

*Structural Analysis Guide*.

*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 Mooney-Rivlin 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. (The default option is

*TBOPT*= MOONEY.)**BOYCE--**Arruda-Boyce model. For

*NPTS*, the default = 3 and the maximum = 3.**References:**Arruda-Boyce Hyperelastic Material in the

*Material Reference*.Arruda-Boyce Hyperelastic Option in the

*Structural Analysis Guide*.**BLATZ --**Blatz-Ko model. For

*NPTS*, the default = 1 and the maximum = 1.**References:**Blatz-Ko Foam Hyperelastic Material in the

*Material Reference*.Blatz-Ko Hyperelastic Option in the

*Structural Analysis Guide*.**ETUBE --**Extended tube model. Five material constants (

*NPTS*= 5) are required.**References:**Extended Tube Material in the

*Material Reference*.Extended Tube Model in the

*Mechanical APDL Theory Reference*.**FOAM --**Hyperfoam (Ogden) model. For

*NPTS*, the default = 1 and the maximum is such that*NTEMP*x*NPTS*x 3 = 1000.**References:**Ogden Compressible Foam Hyperelastic Material in the

*Material Reference*.Ogden Compressible Foam Hyperelastic Option in the

*Structural Analysis Guide*.**GENT --**Gent model. For

*NPTS*, the default = 3 and the maximum = 3.**References:****MOONEY --**Mooney-Rivlin model (default). You can choose a two-parameter Mooney-Rivlin model with

*NPTS*= 2 (default), or a three-, five-, or nine-parameter model by setting*NPTS*equal to one of these values.**References:**Mooney-Rivlin Hyperelastic Material in the

*Material Reference*.Mooney-Rivlin Hyperelastic Option in the

*Structural Analysis Guide*.**NEO --**Neo-Hookean model. For

*NPTS*, the default = 2 and the maximum = 2.**References:**Neo-Hookean Hyperelastic Material in the

*Material Reference*.Neo-Hookean Hyperelastic Option in the

*Structural Analysis Guide*.**OGDEN --**Ogden model. For

*NPTS*, the default = 1 and the maximum is such that*NTEMP*x*NPTS*x 3 = 1000.**References:****POLY --**Polynomial form model. For

*NPTS*, the default = 1 and the maximum is such that*NTEMP*x*NPTS*= 1000.**References:**Polynomial Form Hyperelastic Material in the

*Material Reference*.Polynomial Form Hyperelastic Option in the

*Structural Analysis Guide*.**RESPONSE --**Experimental response function model. For

*NPTS*, the default = 0 and the maximum is such that*NTEMP*x*NPTS*+ 2 = 1000.**References:**Response Function Hyperelastic Material 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 --**Yeoh model. For

*NPTS*, the default = 1 and the maximum is such that*NTEMP*x*NPTS*x 2 = 1000.**References:****USER --**User-defined hyperelastic model. See the ANSYS Guide to User Programmable Features for details.

**References:**User-Defined Hyperelastic Material in the

*Material Reference*.User-Defined Hyperelastic Option in the

*Structural Analysis Guide*.

*NTEMP*:Number of temperatures for which data will be provided. Default = 6. Maximum = 6.

*NPTS*:(Not used for explicit dynamic elements.)

*TBOPT*:Mooney-Rivlin material option, applicable to explicit dynamic elements PLANE162, SHELL163, SOLID164, and SOLID168.

**0 --**Direct input of hyperelastic material constants. This value is the default.

**1 --**Reserved for future use.

**2 --**Material constants to be calculated by the LS-DYNA program from experimental data. This option is only valid for explicit dynamic elements.

**References:**

*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:

**PSE2 --**Pseudo-elastic model with modified Ogden-Roxburgh damage function. Requires

*NPTS*= 3.

**References:**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; Max = 100.

*NPTS:*Number of pairs of Prony series. Default = 1 pair; Max = 100 pairs.

The total number of data points allowed is 1000.

*TBOPT:*Defines the relaxation behavior for viscoelasticity.

**SHEAR--**Shear Prony series.

**BULK --**Bulk Prony series.

**EXPERIMENTAL --**Use complex modulus from experimental data.

**References:**

*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*.**3 --**for

*TBOPT*= 1 or WLF**2 --**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

**1 or WLF --**Williams-Landel-Ferry shift function

**2 or TN --**Tool-Narayanaswamy shift function

**3 or FICT --**Tool-Narayanaswamy with fictive temperature shift function

**100 --**(or USER) User-defined shift function.

**References:**

*NTEMP*:Not used.

*NPTS*:Number of data points to be specified. Default = 20. Maximum = 500.

*TBOPT*:Not used.

**References:**Magnetic Materials in the

*Material Reference*.Additional Guidelines for Defining Regional Material Properties and Real Constants in the

*Low-Frequency Electromagnetic Analysis Guide*.

*NTEMP*:Not used.

*NPTS*:Not used.

*TBOPT*:Not used.

**References:**High-Frequency Electromagnetic Material Models in the

*Material Reference*.

*NTEMP*:Not used.

*NPTS*:Not used.

*TBOPT*:Not used.

**References:**High-Frequency Electromagnetic Material Models in the

*Material Reference*.

*NTEMP:*Not used.

*NPTS:*Not used.

*TBOPT:*Not used for HF118, HF119, and HF120.

Permittivity matrix options for PLANE223, SOLID226, and SOLID227:

**0 --**Permittivity matrix at constant strain [ε

^{S}] (used as supplied)**1 --**Permittivity matrix at constant stress [ε

^{T}] (converted to [ε^{S}] form before use)

**References:**Anisotropic Electric Permittivity Material Model in the

*Material Reference*.

*NTEMP*:Not used.

*NPTS*:Not used.

*TBOPT*:Not used.

**References:**High-Frequency Electromagnetic Materials in the

*Material Reference*.Specifying Material Properties in the

*High-Frequency Electromagnetic Analysis Guide*.

*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.

**References:**FLUID116 in the

*Element Reference*.

*NTEMP*:Not used.

*NPTS*:Not used.

*TBOPT*:Not used.

**References:**High-Frequency Electromagnetic Materials in the

*Material Reference*.Specifying Material Properties in the

*High-Frequency Electromagnetic Analysis Guide*.

*NTEMP*:Not used.

*NPTS*:Not used.

*TBOPT*:Anisotropic relative permeability options:

**0 --**Input permeability matrix.

**1 --**Generate permeability matrix for B-H nonlinear material with uniform dc internal magnetic field

**2 --**Generate permeability matrix for B-H nonlinear material with nonuniform dc internal magnetic field

**References:**High-Frequency Electromagnetic Material Models in the

*Material Reference*.

*NTEMP*:Not used.

*NPTS*:Not used.

*TBOPT*:Piezoelectric matrix options.

**0 --**Piezoelectric stress matrix [e] (used as supplied)

**1 --**Piezoelectric strain matrix [d] (converted to [e] form before use)

**References:**

*NTEMP:*Not used.

*NPTS:*Not used.

*TBOPT:*Piezoresistive matrix options

**0 --**Piezoresistive stress matrix (used as supplied)

**1 --**Piezoresistive strain matrix (used as supplied)

**References:**Piezoresistive Material Model in the

*Material Reference*.Piezoresistive Analysis in the

*Coupled-Field Analysis Guide*.

*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:

**PERM --**Permeability

**BIOT --**Biot coefficient

**References:**Porous Media in the

*Material Reference*.Pore-Fluid-Diffusion-Structural Analysis in the

*Coupled-Field Analysis Guide*.Porous Media Flow in the

*Mechanical APDL Theory Reference*Also see VM260 in the

*Mechanical APDL Verification Manual*.

*NTEMP*:Not used.

*NPTS*:Not used.

*TBOPT*:Explicit spring-damper (discrete) material options.

**0 --**Linear elastic spring (translational or rotational elastic spring). This value is the default.

**1 --**Linear viscous damper (linear translational or rotational damper)

**2 --**Elastoplastic spring (elastoplastic translational or rotational spring with isotropic hardening)

**3 --**Nonlinear elastic spring (nonlinear elastic translational or rotational spring with arbitrary force/displacement response moment/rotation dependency)

**4 --**Nonlinear viscous damper (nonlinear damping with arbitrary force/velocity response moment/rotational velocity dependency)

**5 --**General nonlinear spring (general nonlinear translational or rotational spring with arbitrary loading and unloading definitions)

**6 --**Maxwell viscoelastic spring (Maxwell viscoelastic translational or rotational spring)

**7 --**Inelastic tension or compression-only spring (inelastic tension or compression only, translational or rotational spring)

**References:**Spring-Damper (Discrete) Models in the

*ANSYS LS-DYNA User's Guide*.

*NTEMP*:Not used.

*NPTS*:Not used.

*TBOPT*:Equation of state (explicit dynamic elements only). No default, must specify.

**1 --**Johnson-Cook material model - for strain, strain rate, and temperature dependent impact/forming analyses.

**2 --**Null material model - for allowing equation of state to be considered without computing deviatoric stresses.

**3 --**Zerilli-Armstrong material model - for metal forming processes in which the stress depends on strain, strain rate, and temperature.

**4 --**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).**5 --**Steinberg material model - for modeling high strain rate effects in solid elements with failure.

**References:**

*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.

**References:**FLUID116 in the

*Element Reference*.

*NTEMP*:Not used.

*NPTS*:Not used.

*TBOPT*:Foam material options for explicit dynamics elements (no default - must specify).

**1 --**Rigid, closed cell, low density polyurethane foam material model.

**2 --**Highly compressible urethane foam material model.

**3 --**Energy absorbing foam material model.

**4 --**Crushable foam material model.

**References:**

*NTEMP*:Not used.

*NPTS*:Not used.

*TBOPT*:Not used.

**References:**Pressure Dependent Plasticity Models in the

*ANSYS LS-DYNA User's Guide*.

*NTEMP*:Not used.

*NPTS*:Not used.

*TBOPT*:Plasticity options for explicit dynamics elements (no default - must specify).

**1 --**Isotropic/kinematic hardening model.

**2 --**Strain rate dependent plasticity model used for metal and plastic forming analyses.

**3 --**Anisotropic plasticity model (Barlat and Lian).

**4 --**Strain rate dependent plasticity model used for superplastic forming analyses.

**5 --**Strain rate dependent isotropic plasticity model used for metal and plastic forming analyses.

**6 --**Anisotropic plasticity model (Barlat, Lege, and Brem) used for forming processes.

**7 --**Fully iterative anisotropic plasticity model for explicit shell elements only.

**8 --**Piecewise linear plasticity model for explicit elements only.

**9 --**Elastic-plastic hydrodynamic model for explicit elements only.

**10 --**Transversely anisotropic FLD (flow limit diagram) model for explicit elements only.

**11 --**Modified piecewise linear plasticity model for explicit shell elements only.

**12 --**Elastic viscoplastic thermal model for explicit solid and shell elements only.

**References:**Nonlinear Inelastic Models in the

*ANSYS LS-DYNA User's Guide*.Pressure Dependent Plasticity Models in the

*ANSYS LS-DYNA 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.

*TBOPT*:Fracture criterion option:

**LINEAR --**Linear fracture criterion. Valid when

*NPTS*= 3.**BILINEAR --**Bilinear fracture criterion. Valid when

*NPTS*= 4.**BK --**B-K fracture criterion. Valid when

*NPTS*= 3.**MBK --**Modified B-K (Reeder) fracture criterion. Valid when

*NPTS*= 4.**POWERLAW --**Wu's Power Law fracture criterion. Valid when

*NPTS*= 6.**USER --**User-defined fracture criterion. Valid when

*NPTS*= 20.

**References:**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.

*NPTS*:Number of data points to be specified for a given temperature.

*TBOPT*:Cohesive zone material options.

**EXPO --**Exponential material behavior (valid for interface elements only).

**BILI --**Bilinear material behavior (valid for interface elements only).

**CBDD --**Bilinear material behavior with linear softening characterized by maximum traction and maximum separation (valid for contact elements only).

**CBDE --**Bilinear material behavior with linear softening characterized by maximum traction and critical energy release rate (valid for contact elements only).

**References:**Interface Delamination and Failure Simulation in the

*Structural Analysis Guide*.Cohesive Zone Material Constants in the

*Material Reference*.Cohesive Zone Material (CZM) Model in the

*Mechanical APDL Theory 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 = 4 when

*TBOPT*= MPDG*TBOPT*:Damage initiation definition:

**1 or MPDG --**Progressive damage evolution based on simple instant material stiffness reduction.

**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 = 4 when

*TBOPT*= FCRT.*TBOPT*:Damage initiation definition:

**1 or FCRT --**Define failure criteria as the damage initiation criteria.

**Reference:**

*NTEMP*:Not used.

*NPTS*:Not used.

*TBOPT*:Experimental data type:

**UNITENSION --**Uniaxial tension experimental data.

**UNICOMPRESSION --**Uniaxial compression experimental data.

**UNIAXIAL --**Uniaxial experimental data (combined uniaxial tension and compression).

**BIAXIAL --**Equibiaxial experimental data.

**SHEAR --**Pure shear experimental data (also known as planar tension).

**SSHEAR --**Simple shear experimental data.

**VOLUME --**Volumetric experimental data.

**GMODULUS --**Shear modulus experimental data.

**KMODULUS --**Bulk modulus experimental data.

**EMODULUS --**Tensile modulus experimental data.

**NUXY --**Poisson's ratio experimental data.

**References:**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 field-dependent experimental data.

*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:

**1 --**Define stress-strength limits.

**2 --**Define strain-strength limits.

**References:**

*NTEMP:*Number of temperatures for which data will be provided. Default = 1; Max = 20.

*NPTS:*Number of data points to be specified for a given temperature.

*TBOPT:*Fluid material options:

**LIQUID --**Define material constants for a liquid material.

**GAS --**Define material constants for a gas material.

**PVDATA --**Define pressure-volume data for a fluid material.

**References:**Fluid Material Models in the

*Material Reference*.Fluid Material Models in the

*Mechanical APDL Theory Reference*.

*NTEMP:*Number of temperatures for which data will be provided. Default = 1; Max = 40.

*NTEMP*is not used for the following situations:Isotropic or orthotropic friction defined in terms of field data (

**TBFIELD**command)User-defined friction (

*TBOPT*= USER)

*NPTS:*Number of data points to be specified for user-defined friction (

*TBOPT*= USER). Not used for*TBOPT*= ISO or*TBOPT*= ORTHO.*TBOPT:*Friction options:

**ISO --**Isotropic friction (one coefficient of friction, MU). This option is valid for all 2-D and 3-D contact elements. (Default.)

**ORTHO --**Orthotropic friction (two coefficients of friction, MU1 and MU2). This option is valid for CONTA173, CONTA174, CONTA175, CONTA176, and CONTA177.

**USER --**User defined friction. This option is valid for CONTA171, CONTA172, CONTA173, CONTA174, CONTA175, CONTA176, CONTA177, and CONTA178 elements.

**References:**Contact Friction in the

*Material Reference*.See also the

**TBFIELD**command for more information on 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.

*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.

**PARA --**Gasket material general parameters.

**COMP --**Gasket material compression data.

**LUNL --**Gasket linear unloading data.

**NUNL --**Gasket nonlinear unloading data.

**TSS --**Transverse shear data.

**References:**Gasket Materials in the

*Material Reference*.

*NTEMP*:Not used.

*NPTS*:Number of state variables. Maximum = 1000.

*TBOPT*:Not used.

**References:**User-Defined Material Model and Implicit Creep Equations in the

*Material Reference*.User Defined Material and Implicit Creep Procedure in the

*Structural Analysis Guide*.

*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. Default = 48. The maximum value of

*NPTS*is such that*NTEMP*x*NPTS*= 1000.*TBOPT*:Not used.

**References:**User-Defined Material Model in the

*Material Reference*.User-Defined Material Model in the

*Structural Analysis Guide*.

**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 "Element Support for Material Models" in the *Material Reference*.

For a description of the material model table types (**TB** command *Lab* values), see Material Models in the Mechanical APDL Material Reference.

For a description of data table input required for explicit dynamic materials, see Material Models in the *ANSYS LS-DYNA User's Guide*.

For information about linear material property input, see the **MP** command.

The relationship between SDAMP, **DMPRAT**, and **MP**,BETD is as follows:

Where s is the damping value specified in TB,SDAMP and f is the corresponding frequency.

This command is also valid in SOLUTION.

Command Option Lab | Available Products |

AHYPER | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

ANAN | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

ANEL | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

ANIS | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

BH | MP ME ST <> <> <> <> <> EM <> <> PP <> EME MFS |

BISO | MP ME ST <> PRN <> <> <> <> <> DY PP <> EME MFS |

BKIN | MP ME ST <> PRN <> <> <> <> <> DY PP <> EME MFS |

BOYC | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

CAST | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

CHAB | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

CNDE | MP ME ST <> <> <> <> <> <> EH <> PP <> EME MFS |

CNDM | MP ME ST <> <> <> <> <> <> EH <> PP <> EME MFS |

COMP | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

CONC | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

CREEP | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

CZM | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

DISC | <> <> <> <> <> <> <> <> <> <> DY PP <> <> <> |

DP | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

DPER | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

EDP | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

ELASTIC | MP ME ST PR PRN <> <> <> <> <> DY PP <> EME MFS |

EOS | <> <> <> <> <> <> <> <> <> <> DY PP <> <> <> |

EVIS | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

FCON | MP ME ST PR PRN <> <> <> <> <> DY PP <> EME MFS |

FOAM | <> <> <> <> <> <> <> <> <> <> DY PP <> <> <> |

FRIC | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

GASKET | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

GCAP | <> <> <> <> <> <> <> <> <> <> DY PP <> <> <> |

HFLM | MP ME ST PR PRN <> <> <> <> <> DY PP <> EME MFS |

HILL | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

HONEY | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

HYPER | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

HYPER - MOONEY (NPTS = 2) | MP ME ST <> PRN <> <> <> <> <> DY PP <> EME MFS |

HYPER - OGDEN | MP ME ST <> PRN <> <> <> <> <> DY PP <> EME MFS |

HYPER - NEO | MP ME ST <> PRN <> <> <> <> <> DY PP <> EME MFS |

KINH | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

JOIN | MP ME ST PR PRN <> <> <> <> <> DY PP <> EME MFS |

MELA | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

MISO | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

MKIN | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

MOON | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

MUR | MP ME ST <> <> <> <> <> <> EH <> PP <> EME MFS |

NL | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

NLIS | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

PFLO | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

PIEZ | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

PLASTIC | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

PLAW | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

PROONY | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

PZRS | MP ME ST <> <> <> <> <> <> <> <> PP <> EME MFS |

RATE | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

SDAMP | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

SHIFT | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

SMA | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

STATE | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

SWELL | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

UNIAXIAL | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |

USER | MP ME ST <> <> <> <> <> <> <> DY PP <> EME MFS |