You use the Edit Material dialog box to create a plastic material and to specify its material properties. You can create the following plastic material models:
Classical metal plasticity; see “Defining classical metal plasticity”
Cap plasticity; see “Defining cap plasticity”
Cast iron plasticity; see “Defining cast iron plasticity”
Clay plasticity; see “Defining clay plasticity”
Concrete damaged plasticity; see “Defining concrete damaged plasticity”
Concrete smeared cracking; see “Defining concrete smeared cracking”
Crushable foam plasticity; see “Defining crushable foam plasticity”
Drucker-Prager plasticity; see “Defining Drucker-Prager plasticity”
Mohr-Coulomb plasticity; see “Defining Mohr-Coulomb plasticity”
Porous metal plasticity; see “Defining porous metal plasticity”
Creep; see “Defining a creep law”
Swelling; see “Defining swelling”
Viscous; see “Defining the viscous component of a two-layer viscoplasticity model”
The classical metal plasticity model allows you to define the yield and inelastic flow of a metal at relatively low temperatures, where loading is relatively monotonic and creep effects are unimportant. For more information, see “Classical metal plasticity,” Section 23.2.1 of the Abaqus Analysis User's Guide.
When you use the Edit Material dialog box to define the classical plastic behavior of a material, you must select one of the following options for specifying hardening behavior:
Select Isotropic to model hardening where the yield surface changes size uniformly in all directions such that the yield stress increases (or decreases) in all stress directions as plastic straining occurs. See “Using an isotropic hardening model to define classical metal plasticity” for detailed instructions.
Select Kinematic to model the cyclic loading of a material with a constant rate of hardening. See “Using a linear kinematic cyclic hardening model to define classical metal plasticity” for detailed instructions.
Select Johnson-Cook to model isotropic hardening in Abaqus/Explicit, where the yield stress is provided as an analytical function of equivalent plastic strain, strain rate, and temperature. See “Using the Johnson-Cook hardening model to define classical metal plasticity” for detailed instructions.
Select User to described the yield stress for isotropic hardening through user subroutine UHARD. See “Specifying user subroutine UHARD to define classical metal plasticity” for detailed instructions.
Select Combined to model the cyclic loading of a material with nonlinear isotropic/kinematic hardening. See “Using a nonlinear isotropic/kinematic cyclic hardening model to define classical metal plasticity” for detailed instructions.
The isotropic hardening model is useful for cases involving gross plastic straining or for cases where the straining at each point is essentially in the same direction in strain space throughout the analysis.
To define an isotropic hardening model:
From the menu bar in the Edit Material dialog box, select Mechanical
PlasticityPlastic.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Click the arrow to the right of the Hardening field, and select Isotropic.
Toggle on Use strain-rate-dependent data if you want enter test data showing yield stress values versus equivalent plastic strain at different equivalent plastic strain rates.
A Rate column appears in the Data table.
Alternatively, if you want to define strain rate dependence using yield stress ratios, you must select Rate Dependent from the Suboptions menu. See “Defining rate-dependent yield with yield stress ratios” for details. For background information on rate dependence, see “Rate-dependent yield,” Section 23.2.3 of the Abaqus Analysis User's Guide.
Toggle on Use temperature-dependent data to define behavior data that depend on temperature.
A column labeled Temp appears in the Data table.
To define behavior data that depend on field variables, click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables.
Enter the following data in the Data table:
Yield Stress
The stress at which yield is initiated.
Plastic Strain
Plastic strain.
Rate
Equivalent plastic strain rate, 
, for which the stress-strain curve applies.
Temp
Temperature.
Field n
Predefined field variables.
If desired, use the Suboptions menu to enter additional data. See the following sections for details:
Click OK to create the material and to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
Use the linear kinematic model to define a constant rate of cyclic hardening. See “Models for metals subjected to cyclic loading,” Section 23.2.2 of the Abaqus Analysis User's Guide, for more information.
To define a linear kinematic hardening model:
From the menu bar in the Edit Material dialog box, select MechanicalPlasticityPlastic.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Click the arrow to the right of the Hardening field, and select Kinematic.
Toggle on Use temperature-dependent data to define behavior data that depend on temperature.
A column labeled Temp appears in the Data table.
Enter the following data in the Data table:
Yield Stress
The stress at which yield is initiated.
Plastic Strain
Plastic strain.
Temp
Temperature.
If desired, use the Suboptions menu to enter additional data. See the following sections for details:
Click OK to create the material and to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
The Johnson-Cook plasticity model is particularly suited to model high-strain-rate deformation of metals. This model is a particular type of Mises plasticity that includes analytical forms of the hardening law and rate dependence. It is generally used in adiabatic transient dynamic analysis. For more information, see “Johnson-Cook plasticity,” Section 23.2.7 of the Abaqus Analysis User's Guide.
To define a Johnson-Cook hardening model:
From the menu bar in the Edit Material dialog box, select MechanicalPlasticityPlastic.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Click the arrow to the right of the Hardening field, and select Johnson-Cook.
Enter the following data in the Data table:
A, B, n, and m
Material parameters measured at or below the transition temperature.
Melting Temp
Melting temperature, 
, above which the material is melted and behaves like a fluid.
Transition Temp
Transition temperature, 
. There is no temperature dependence on the expression of the yield stress at or below the transition temperature.
If desired, use the Suboptions menu to enter additional data. See the following sections for details:
Click OK to create the material and to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
User subroutine UHARD allows you to define the yield surface size and hardening parameters for isotropic plasticity or combined hardening models.
To define classical metal plasticity with user subroutine UHARD:
From the menu bar in the Edit Material dialog box, select MechanicalPlasticityPlastic.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Click the arrow to the right of the Hardening field, and select User.
In the Data table, enter the number of Hardening Properties needed as data in user subroutine UHARD.
Click OK to create the material and to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
The evolution law of this model consists of two components:
A nonlinear kinematic hardening component, which describes the translation of the yield surface in stress space through the backstress, 
.
An isotropic hardening component, which describes the change of the equivalent stress defining the size of the yield surface, 
, as a function of plastic deformation.
You can define the kinematic hardening component by selecting Combined from the list of Hardening options in the Edit Material dialog box and entering the required data.
You can define the isotropic hardening component by selecting Cyclic Hardening from the Suboptions menu and entering data in the Suboption Editor that appears.
For more information on cyclic hardening, see “Models for metals subjected to cyclic loading,” Section 23.2.2 of the Abaqus Analysis User's Guide.
To define a nonlinear isotropic/kinematic hardening model:
From the menu bar in the Edit Material dialog box, select MechanicalPlasticityPlastic.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Click the arrow to the right of the Hardening field, and select Combined.
Click the arrow to the right of the Data type field, and specify how you want to define the kinematic hardening component of the model:
Select Half Cycle to provide stress-strain data obtained from the first half cycle of a unidirectional tension or compression experiment.
Select Parameters to specify the kinematic hardening parameters 
and 
directly.
Select Stabilized to provide stress-strain data obtained from the stabilized cycle of a specimen that is subjected to symmetric strain cycles.
To specify the number of backstresses to include in the model, click the arrows to the right of the Number of backstresses field. The default number of backstresses is 1. The maximum number of backstresses allowed is 10.
If you selected Parameters from the list of Data type options, additional columns appear in the table to specify the kinematic hardening parameters for multiple backstresses.
Toggle on Use temperature-dependent data to define behavior data that depend on temperature.
A column labeled Temp appears in the Data table.
To define behavior data that depend on field variables, click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables.
If you selected Stabilized from the list of Data type options, you can choose to toggle on Use strain-range-dependent data. This option is useful if the shapes of the stress-strain curves are significantly different for different strain ranges.
In the Data table, enter the data relevant to your Data type selection (not all of the following parameters will apply):
Yield Stress
The stress at which yield is initiated.
Plastic Strain
Plastic strain.
Yield Stress At Zero Plastic Strain
Yield stress at zero plastic strain, 
.
Kinematic Hard Parameter C1
Kinematic hardening parameter, 
.
Gamma 1
Kinematic hardening parameter, 
.
Kinematic Hard Parameter Ck and Gamma k
Kinematic hardening parameters and for multiple backstresses.
Temp
Temperature.
Field n
Predefined field variables.
Strain Range
The strain range at which the stress-strain curve is obtained.
To define the isotropic hardening component of the model, select Cyclic Hardening from the Suboptions menu, and enter the required data in the Suboption Editor that appears. See “Defining the isotropic hardening component of a nonlinear isotropic/kinematic hardening model” for details.
If desired, use other options from the Suboptions menu to enter additional data. See the following sections for details:
Click OK to create the material and to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
The Suboption Editor allows you to define the evolution of the elastic domain for the nonlinear isotropic/kinematic hardening model. For more information, see the following sections:
“Models for metals subjected to cyclic loading,” Section 23.2.2 of the Abaqus Analysis User's Guide
“Using a nonlinear isotropic/kinematic cyclic hardening model to define classical metal plasticity”
To define the isotropic hardening component:
Create a material model as described in “Using a nonlinear isotropic/kinematic cyclic hardening model to define classical metal plasticity.”
From the Suboptions menu in the Edit Material dialog box, select Cyclic Hardening.
A Suboption Editor appears.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
To define data that depend on field variables, click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables.
Specify how you want to define the isotropic hardening component:
Toggle on Use parameters if you want to enter the material parameters of the exponential law.
Toggle off Use parameters if you want to define the evolution of the yield surface size as a function of the equivalent plastic strain in tabular form.
If you toggled on Use parameters, enter the following data in the Data table:
Equiv Stress
Equivalent stress defining the size of the elastic range at zero plastic strain.
Q-infinity
Isotropic hardening parameter, 
.
Hardening Param b
Isotropic hardening parameter, b.
Temp
Temperature.
Field n
Predefined field variables.
If you toggled off Use parameters, enter the following data in the Data table:
Equiv Stress
Equivalent stress defining the size of the elastic range.
Equiv Plastic Strain
Equivalent plastic strain.
Temp
Temperature.
Field n
Predefined field variables.
You may need to expand the dialog box to see all the columns in the Data table. For detailed information on how to enter data, see “Entering tabular data,” Section 3.2.7.
Click OK to return to the Edit Material dialog box.
Abaqus allows you to define a material's yield behavior accurately when the yield strength depends on the rate of straining and the anticipated strain rates are significant. You can define strain rate dependence in two ways:
Enter hardening curves at different strain rates directly, as described in the following sections:
Define yield stress ratios to specify the rate dependence independently, as described in the procedure below.
To define rate dependent yield using stress ratios:
Create a material model as described in described in one of the following sections:
From the Suboptions menu in the Edit Material dialog box, select Rate Dependent.
A Suboption Editor appears.
Click the arrow to the right of the Hardening field, and select a method for defining hardening dependencies:
Select Power Law to define yield stress ratios with the Cowper-Symonds overstress law.
Select Tabular to enter yield stress ratios directly in tabular form as a function of equivalent plastic strain rates.
Select Johnson-Cook to use an analytical Johnson-Cook form to define R.
If applicable, toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
If applicable, click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
If you selected Power Law from the list of Hardening options, enter the following data in the Data table:
Mulitiplier
Material parameter, D.
Exponent
Material parameter, n.
Temp
Temperature.
Field n
Predefined field variables.
If you selected Yield Ratio from the list of Hardening options, enter the following data in the Data table:
Yld Stress Ratio
Yield stress ratio, 
.
Eq Plastic Strain Rate
Equivalent plastic strain rate, (or 
, the absolute value of the axial plastic strain rate in uniaxial compression, for the crushable foam model).
Temp
Temperature.
Field n
Predefined field variables.
If you selected Johnson-Cook from the list of Hardening options, enter the following data in the Data table:
C
Material constant, C, which is independent of temperature and field variables.
Epsilon dot zero
Material constant, 
, which is independent of temperature and field variables.
For detailed information on how to enter data, see “Entering tabular data,” Section 3.2.7.
Click OK to return to the Edit Material dialog box.
Abaqus provides an anisotropic yield and creep model for materials that exhibit different yield or creep behavior in different directions. You can define anisotropic yield or creep by specifying stress ratios that are applied in Hill's potential function. For more information, see “Anisotropic yield/creep,” Section 23.2.6 of the Abaqus Analysis User's Guide.
To define anisotropic yield or creep:
Create a material model as described in one of the following sections
“Using an isotropic hardening model to define classical metal plasticity”
“Using a linear kinematic cyclic hardening model to define classical metal plasticity”
“Using a nonlinear isotropic/kinematic cyclic hardening model to define classical metal plasticity”
“Defining the viscous component of a two-layer viscoplasticity model”
From the Suboptions menu in the Edit Material dialog box, select Potential.
A Suboption Editor appears.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
Enter the following data in the Data table:
R11, R22, R33, R12, R13, and R23
Yield or creep stress ratios.
Temp
Temperature.
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
The ORNL constitutive model in Abaqus/Standard applies to Types 304 and 316 stainless steel, as specified in nuclear standard NE F9–5T(1981). The constitutive theory is uncoupled into a rate-independent plasticity response and a rate-dependent creep response, each of which is governed by a separate constitutive law. For more information, see “ORNL – Oak Ridge National Laboratory constitutive model,” Section 23.2.12 of the Abaqus Analysis User's Guide, and “ORNL constitutive theory,” Section 4.3.8 of the Abaqus Theory Guide.
To specify the constitutive model developed by Oak Ridge National Laboratory:
Create a material model as described in one of the following sections:
From the Suboptions menu in the Edit Material dialog box, select Ornl.
A Suboption Editor appears.
In the Saturation rates for kinematic shift field, enter a value for A, the parameter equal to the saturation rates for kinematic shift caused by creep strain. This parameter is defined by Equation (15) of Section 4.3.3--3 of the Nuclear Standard. The default value is 0.3. Set A=0.0 to use the 1986 revision of the Standard.
In the Rate of kinematic shift wrt creep strain field, enter a value for H, the parameter equal to the rate of kinematic shift with respect to creep strain. This parameter is defined by Equation (7) of Section 4.3.2–1 of the Nuclear Standard. Set H=0.0 to use the 1986 revision of the Standard. If you omit this parameter, Abaqus determines the value of H according to Section 4.3.3–3 of the 1981 revision of the Standard.
If desired, toggle on Invoke reset procedure to invoke the optional 
reset procedure described in Section 4.3.5 of the Nuclear Standard.
Click OK to return to the Edit Material dialog box.
You can use the Suboption editor to specify the tenth-cycle yield stress and hardening values for the ORNL constitutive model. This option is relevant only if you also follow the procedure described in “Using the Oak Ridge National Laboratory (ORNL) constitutive model in plasticity and creep calculations.”
To specify the cycled yield stress data for the ORNL model:
Create a material model as described in “Using a linear kinematic cyclic hardening model to define classical metal plasticity.”
From the Suboptions menu in the Edit Material dialog box, select Cycled Plastic.
A Suboption Editor appears.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
In the Data table, enter values for the yield stress, plastic strain, and, if applicable, temperature.
For detailed information on how to enter data, see “Entering tabular data,” Section 3.2.7.
Click OK to return to the Edit Material dialog box.
When the temperature of a material point exceeds its annealing temperature, Abaqus assumes that the material point loses its hardening memory. You can specify an annealing temperature and, if desired, define it in terms of field variables. See “Annealing or melting,” Section 23.2.5 of the Abaqus Analysis User's Guide, for more information.
To specify an annealing temperature:
Create a material model as described in one of the following sections
“Using an isotropic hardening model to define classical metal plasticity”
“Using a linear kinematic cyclic hardening model to define classical metal plasticity”
“Using a nonlinear isotropic/kinematic cyclic hardening model to define classical metal plasticity”
“Using the Johnson-Cook hardening model to define classical metal plasticity”
From the Suboptions menu in the Edit Material dialog box, select Anneal Temperature.
A Suboption Editor appears.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the anneal temperature depends.
Enter the following data in the Data table:
Anneal Temperature
Value of the annealing temperature, 
.
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
Abaqus allows you to define yield surface parameters for elastic-plastic materials that use the modified Drucker-Prager\Cap plasticity model. See “Modified Drucker-Prager/Cap model,” Section 23.3.2 of the Abaqus Analysis User's Guide, for more information.
You can use the modified Drucker-Prager/Cap plasticity model to simulate geological materials that exhibit pressure-dependent yield. The addition of a cap yield surface helps control volume dilatancy when the material yields in shear and provides an inelastic hardening mechanism to represent plastic compaction. You can also define inelastic time-dependent (creep) behavior coupled with the plastic behavior in an Abaqus/Standard analysis.
For more information on cap plasticity, see “Modified Drucker-Prager/Cap model,” Section 23.3.2 of the Abaqus Analysis User's Guide.
To define cap plasticity:
From the menu bar in the Edit Material dialog box, select MechanicalPlasticityCap Plasticity.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
In the Data table, enter the following data:
Material Cohesion
Material cohesion, d, in the p–t plane (Abaqus/Standard) or in the p–q plane (Abaqus/Explicit). (Units of FL–2.)
Angle of Friction
Material angle of friction, 
, in the p–t plane (Abaqus/Standard) or in the p–q plane (Abaqus/Explicit). Enter the value in degrees.
Cap Eccentricity
Cap eccentricity parameter, R. Its value must be greater than zero (typically 
).
Init Yld Surf Pos
Initial cap yield surface position, 
.
Transition Surf Rad
Transition surface radius parameter, . Its value should be a small number compared to unity. If you leave this field blank, the default is 0.0 (i.e., no transition surface). If you include creep properties in the material model, you must set equal to zero.
Flow Stress Ratio
The ratio of the flow stress in triaxial tension to the flow stress in triaxial compression, K. The value of K should be such that 
. If you leave this field blank or enter a value of 0.0, Abaqus uses a value of 1.0 by default. If you include creep properties in the material model, you should set K equal to 1.0. This parameter applies only to Abaqus/Standard analyses.
Temp
Temperature.
Field n
Predefined field variables.
To define the hardening part of the cap plasticity model, select Cap Hardening from the Suboptions menu. See “Defining hardening parameters for a cap plasticity model” for detailed instructions.
If you want to specify cap creep behavior, select one of the following options from the Suboptions menu:
Select Cap Creep Cohesion to choose a cohesion creep mechanism that follows the type of plasticity active in the shear-failure plasticity.
Select Cap Creep Consolidation to choose a consolidation mechanism that follows the type of plasticity active in the cap plasticity region.
Click OK to create the material and to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
The hardening curve specified for this model interprets yielding in the hydrostatic pressure sense: the hydrostatic pressure yield stress is defined as a tabular function of the volumetric inelastic strain, and, if desired, a function of temperature and other predefined field variables. The range of values for which you define 
should be sufficient to include all values of effective pressure stress that the material will be subjected to during the analysis.
See “Modified Drucker-Prager/Cap model,” Section 23.3.2 of the Abaqus Analysis User's Guide, for more information.
To define cap hardening:
Create a material model as described in “Specifying cap plasticity behavior.”
From the Suboptions menu in the Edit Material dialog box, select Cap Hardening.
A Suboption Editor appears.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
In the Data table, enter the following data:
Yield Stress
Hydrostatic pressure yield stress. (The initial tabular value must be greater than zero, and values must increase with increasing volumetric inelastic strain.)
Vol Plas Strain
Absolute value of the corresponding volumetric inelastic strain.
Temp
Temperature.
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
The cap creep model has two possible mechanisms that are active in different loading regions: one is a cohesion mechanism, which follows the type of plasticity active in the shear-failure plasticity region, and the other is a consolidation mechanism, which follows the type of plasticity active in the cap plasticity region.
For more information, see “Creep formulation” in “Modified Drucker-Prager/Cap model,” Section 23.3.2 of the Abaqus Analysis User's Guide.
To define cap creep:
Create a material model as described in “Specifying cap plasticity behavior.”
From the Suboptions menu in the Edit Material dialog box, select either Cap Creep Cohesion or Cap Creep Consolidation. (See “Creep formulation” in “Modified Drucker-Prager/Cap model,” Section 23.3.2 of the Abaqus Analysis User's Guide, for detailed information on the two creep mechanisms.)
A Suboption Editor appears.
Click the arrow to the right of the Law field, and select the creep law option of your choice:
Select Strain to choose a strain hardening power law.
Select Time to choose a time hardening power law
Select SinghM to choose a Singh-Mitchell type law.
Select User to specify the creep law with user subroutine CREEP.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
If you selected either the Strain or the Time creep law option, enter the following data in the Data table:
A, n, and m
Creep material parameters.
Temp
Temperature.
Field n
Predefined field variables.
If you selected the SinghM creep law option, enter the following data in the Data table:
A, alpha, m, and t1
Creep material parameters A, , m, and 
.
Temp
Temperature.
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
The cast iron plasticity model describes the mechanical behavior of gray cast iron, a material whose microstructure consisting of graphite flakes in a steel matrix. The model definition includes the plastic Poisson's ratio and information on hardening under compression and tension. See “Cast iron plasticity,” Section 23.2.10 of the Abaqus Analysis User's Guide, for more information.
To define cast iron plasticity:
From the menu bar in the Edit Material dialog box, select MechanicalPlasticityCast Iron Plasticity.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Display the Plasticity tabbed page, and do the following:
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
Enter the following data in the Data table:
Plastic Poisson's Ratio
Value of the plastic “Poisson's ratio,” 
, where 
. (Dimensionless.) The default value is 
.
Temp
Temperature, 
.
Field n
Predefined field variables.
Display the Compression Hardening tabbed page, and do the following:
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
Enter the following data in the Data table:
Sigmac
Yield stress in compression, 
.
Epsilonc
Absolute value of the corresponding plastic strain. (The first tabular value entered must always be zero.)
Temp
Temperature.
Field n
Predefined field variables.
Display the Tension Hardening tabbed page, and do the following:
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
Enter the following data in the Data table:
Sigmat
Yield stress in uniaxial tension, 
.
Epsilont
Corresponding plastic strain. (The first tabular value entered must always be zero.)
Temp
Temperature.
Field n
Predefined field variables.
Click OK to create the material and to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
The clay plasticity model allows you to specify the plastic part of the material behavior for elastic-plastic materials that use the extended Cam-clay plasticity model. See “Critical state (clay) plasticity model,” Section 23.3.4 of the Abaqus Analysis User's Guide, for more details.
The Abaqus/Standard clay plasticity model describes the inelastic response of cohesionless soils. This model provides a reasonable match to the experimentally observed behavior of saturated clays. You can define the inelastic material behavior by a yield function that depends on the three stress invariants, an associated flow assumption to define the plastic strain rate, and a strain hardening theory that changes the size of the yield surface according to the inelastic volumetric strain.
For more information, see “Critical state (clay) plasticity model,” Section 23.3.4 of the Abaqus Analysis User's Guide.
To define clay plasticity:
From the menu bar in the Edit Material dialog box, select MechanicalPlasticityClay Plasticity.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Click the arrow to the right of the Hardening field, and select the hardening law form of your choice:
Select Exponential to specify an exponential hardening/softening law.
Select Tabular to specify a piecewise linear hardening/softening relationship.
If you selected the Exponential form of the hardening law, you have the option of entering a value for Intercept. This parameter corresponds to 
, the intercept of the virgin consolidation line with the void ratio axis in a plot of void ratio versus the logarithm of pressure stress.
If you specify a value for Intercept, Abaqus ignores any value specified for the initial yield surface size, 
, in the Data table.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
If you selected the Exponential form of the hardening law, enter the following data in the Data table:
Log Plas Bulk Mod
Logarithmic plastic bulk modulus, 
(dimensionless).
Stress Ratio
Stress ratio at critical state, M.
Init Yld Surf Size
Initial yield surface size, (units of FL–2). Abaqus ignores this data item if you have specified a value for Intercept.
Wet Yld Surf Size
Parameter defining the size of the yield surface on the “wet” side of critical state, . If this value is omitted or set to zero, a value of 1.0 is assumed.
Flow Stress Ratio
Ratio of the flow stress in triaxial tension to the flow stress in triaxial compression, K. . If this value is left blank or set to zero, a value of 1.0 is assumed.
Temp
Temperature.
Field n
Predefined field variables.
If you selected the Tabular form of the hardening law, enter the following data in the Data table:
Stress Ratio
Stress ratio at critical state, M.
Init Vol Plas Strain
Initial volumetric plastic strain, 
corresponding to 
.
Wet Yld Surf Size
Parameter defining the size of the yield surface on the “wet” side of critical state, . If this value is omitted or set to zero, a value of 1.0 is assumed.
Flow Stress Ratio
Ratio of the flow stress in triaxial tension to the flow stress in triaxial compression, K. . If this value is left blank or set to zero, a value of 1.0 is assumed.
Temp
Temperature.
Field n
Predefined field variables.
If you selected the Tabular form of the hardening law, select Compressive Clay Hardening from the Suboptions menu to provide the hydrostatic compression yield stress as a function of volumetric plastic strain to define piecewise linear hardening/softening of the Cam-clay plasticity yield surface. See “Defining compressive clay hardening for a clay plasticity model” for detailed instructions.
If you selected the Tabular form of the hardening law, select Tensile Clay Hardening from the Suboptions menu to provide the hydrostatic tension yield stress as a function of volumetric plastic strain to define piecewise linear hardening/softening of the Cam-clay plasticity yield surface. See “Defining tensile clay hardening for a clay plasticity model” for detailed instructions.
If desired, select Potential from the Suboptions menu to specify anisotropic yield behavior. See “Defining anisotropic yield and creep” for more information.
If desired, select Softening Regularization from the Suboptions menu to specify a regularization scheme to mitigate potential mesh independence of the results. See “Specifying softening regularization for a clay plasticity model” for detailed instructions.
Click OK to create the material and to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
The Suboption Editor allows you to provide the hydrostatic compression yield stress as a function of volumetric plastic strain to define piecewise linear hardening/softening of the Cam-clay plasticity yield surface. For more information on this form of the hardening law, see “Piecewise linear form” in “Critical state (clay) plasticity model,” Section 23.3.4 of the Abaqus Analysis User's Guide.
To define compressive clay hardening:
Create a material model as described in “Specifying clay plasticity behavior.”
From the Suboptions menu in the Edit Material dialog box, select Compressive Clay Hardening.
A Suboption Editor appears.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
In the Data table, enter the following data:
Yield Stress
Value of the hydrostatic pressure stress at yield, 
. is given as a positive value and must increase with increasing volumetric plastic strain.
Vol Plas Strain
Absolute value of the corresponding compressive volumetric plastic strain. (The first tabular value must always be zero.)
Temp
Temperature.
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
The Suboption Editor allows you to provide the hydrostatic tensile yield stress as a function of volumetric plastic strain to define piecewise linear hardening/softening of the Cam-clay plasticity yield surface. For more information on this form of the hardening law, see “Piecewise linear form” in “Critical state (clay) plasticity model,” Section 23.3.4 of the Abaqus Analysis User's Guide.
To define tensile clay hardening:
Create a material model as described in “Specifying clay plasticity behavior.”
From the Suboptions menu in the Edit Material dialog box, select Tensile Clay Hardening.
A Suboption Editor appears.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
In the Data table, enter the following data:
Yield Stress
Value of the hydrostatic pressure stress at yield, 
. can be zero or a negative value and must decrease with increasing volumetric plastic strain.
Vol Plas Strain
Absolute value of the corresponding compressive volumetric plastic strain. (The first tabular value must always be zero.)
Temp
Temperature.
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
The Suboption Editor allows you to specify a regularization scheme to mitigate potential mesh dependence of results in the Cam-clay plasticity model in the event that it exhibits strain localization with increasing plastic deformation For more information, see “Softening regularization” in “Critical state (clay) plasticity model,” Section 23.3.4 of the Abaqus Analysis User's Guide.
To define softening regularization:
Create a material model as described in “Specifying clay plasticity behavior.”
From the Suboptions menu in the Edit Material dialog box, select Softening Regularization.
A Suboption Editor appears.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
In the Data table, enter the following data:
Crack Band Length
Crack band length, 
. This value must be greater than zero.
Exponent
Exponent, 
. This value must be greater than zero.
Bound
Bound on the magnitude of regularization, 
. This value must be greater than zero.
Temp
Temperature.
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
The concrete damaged plasticity model provides a general capability for modeling concrete and other quasi-brittle materials in all types of structures. This model uses concepts of isotropic damaged elasticity in combination with isotropic tensile and compressive plasticity to represent the inelastic behavior of concrete. See “Concrete damaged plasticity,” Section 23.6.3 of the Abaqus Analysis User's Guide, for more information.
The concrete damaged plasticity model is based on the assumption of scalar (isotropic) damage and is designed for applications in which the concrete is subjected to arbitrary loading conditions, including cyclic loading. The model takes into consideration the degradation of the elastic stiffness induced by plastic straining both in tension and compression. It also accounts for stiffness recovery effects under cyclic loading.
For more information, see “Concrete damaged plasticity,” Section 23.6.3 of the Abaqus Analysis User's Guide.
To define concrete damaged plasticity:
From the menu bar in the Edit Material dialog box, select MechanicalPlasticityConcrete Damaged Plasticity.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Click the Plasticity tab, if necessary, to display the Plasticity tabbed page.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
Enter the following data in the Data table:
Dilation Angle
Dilation angle, 
, in the p–q plane. Enter the value in degrees.
Eccentricity
Flow potential eccentricity, 
. The eccentricity is a small positive number that defines the rate at which the hyperbolic flow potential approaches its asymptote. The default is 
.
fb0/fc0
, the ratio of initial equibiaxial compressive yield stress to initial uniaxial compressive yield stress. The default value is 
K
, the ratio of the second stress invariant on the tensile meridian, 
, to that on the compressive meridian, 
, at initial yield for any given value of the pressure invariant p such that the maximum principal stress is negative, 
. It must satisfy the condition 
. The default value is 
.
Viscosity Parameter
Viscosity parameter, 
, used for the visco-plastic regularization of the concrete constitutive equations in Abaqus/Standard analyses. This parameter is ignored in Abaqus/Explicit. The default value is 
. (Units of 
.)
Temp
Temperature.
Field n
Predefined field variables.
Click the Compressive Behavior tab to display the Compressive Behavior tabbed page. (For information on compressive hardening, see “Defining compressive behavior” in “Concrete damaged plasticity,” Section 23.6.3 of the Abaqus Analysis User's Guide.)
Toggle on Use strain-rate-dependent data if the compressive stress data are a function of strain rate.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
Enter the following data in the Data table:
Yield Stress
Yield stress in compression, 
. (Units of 
.)
Inelastic Strain
Inelastic (crushing) strain, 
.
Rate
Inelastic (crushing) strain rate, 
. (Units of 
.)
Temp
Temperature.
Field n
Predefined field variables.
If desired, select Compression Damage from the Suboptions menu to specify damage in tabular form. (If you omit damage data, the model behaves as a plasticity model.) See “Defining concrete compression damage” for details.
Click the Tensile Behavior tab to display the Tensile Behavior tabbed page. (For information on tension stiffening, see “Defining tension stiffening” in “Concrete damaged plasticity,” Section 23.6.3 of the Abaqus Analysis User's Guide.)
Click the arrow to the right of the Type field, and select a method for defining the postcracking behavior:
Select Strain to specify the postcracking behavior by entering the postfailure stress/cracking-strain relationship.
Select Displacement to define the postcracking behavior by entering the postfailure stress/cracking-displacement relationship.
Select GFI to define the postcracking behavior by entering the failure stress and the fracture energy.
Toggle on Use strain-rate-dependent data if the postcracking stress depends on strain rate.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
In the Data table, enter the data relevant to your Type choice from Step 13 (not all of the following will apply):
Yield Stress
If you selected Strain or Displacement from the list of Type options, enter the remaining direct stress after cracking, 
. (Units of .)
If you selected GFI from the list of Type options, enter the failure stress, 
. (Units of .)
Cracking Strain
Direct cracking strain, 
.
Displacement
Direct cracking displacement, 
. (Units of L.)
Fracture Energy
Fracture energy, 
. (Units of 
.)
Rate
If you selected Strain from the list of Type options, enter the direct cracking strain rate, 
. (Units of .)
If you selected Displacement or GFI from the list of Type options, enter the direct cracking displacement rate, 
. (Units of 
.)
Temp
Temperature.
Field n
Predefined field variables.
If desired, select Tension Damage from the Suboptions menu to specify damage in tabular form. (If you omit damage data, the model behaves as a plasticity model.) See “Defining concrete tension damage” for details.
Click OK to create the material and to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
You can define the uniaxial compression damage variable, 
, as a tabular function of inelastic (crushing) strain. For more information, see “Defining damage and stiffness recovery” in “Concrete damaged plasticity,” Section 23.6.3 of the Abaqus Analysis User's Guide.
To define compression damage:
Create a material model as described in “Defining a concrete damaged plasticity model.”
From the Suboptions menu on the Compressive Behavior tabbed page, select Compression Damage.
A Suboption Editor appears.
In the Tension recovery field, enter a value for the stiffness recovery factor 
, which determines the amount of tension stiffness that is recovered as the loading changes from compression to tension.
If 
, the material fully recovers the tensile stiffness; if 
, there is no stiffness recovery. Intermediate values of 
result in partial recovery of the tensile stiffness. The default value is 0.0.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
Enter the following data in the Data table:
Damage Parameter
Compressive damage variable, .
Inelastic Strain
Inelastic (crushing) strain, .
Temp
Temperature.
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
You can define the uniaxial tension damage variable, 
, as a tabular function of either cracking strain or cracking displacement.For more information, see “Defining damage and stiffness recovery” in “Concrete damaged plasticity,” Section 23.6.3 of the Abaqus Analysis User's Guide.
To define tensile damage:
Create a material model as described in “Defining a concrete damaged plasticity model.”
From the Suboptions menu in the Tensile Behavior tabbed page, select Tension Damage.
A Suboption Editor appears.
Click the arrow to the right of the Type field, and select a method for defining the tensile damage variable:
Select Strain to specify the tensile damage variable as a function of cracking strain.
Select Displacement to specify the tensile damage variable as a function of cracking displacement.
In the Compression recovery field, enter a value for the stiffness recovery factor, 
, which determines the amount of compression stiffness that is recovered as the loading changes from tension to compression.
If 
, the material fully recovers the compressive stiffness; if 
, there is no stiffness recovery. Intermediate values of 
result in partial recovery of the compressive stiffness. The default value is 
, which corresponds to the assumption that as cracks close the compressive stiffness is unaffected by tensile damage.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
In the Data table, enter the data relevant to your Type selection from Step 3 (not all of the following will apply):
Damage Parameter
Tensile damage variable, .
Cracking Strain
Direct cracking strain, .
Displacement
Direct cracking displacement, . (Units of L.)
Temp
Temperature.
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
You can use the concrete smeared cracking model to define the properties of plain concrete outside the elastic range in an Abaqus/Standard analysis. For more information, see “Concrete smeared cracking,” Section 23.6.1 of the Abaqus Analysis User's Guide.
The concrete smeared cracking model allows you to define concrete behavior for relatively monotonic loadings under fairly low confining pressures. Abaqus assumes that cracking is the most important aspect of the behavior, and representation of cracking and postcracking behavior dominates the modeling. For more information, see “Concrete smeared cracking,” Section 23.6.1 of the Abaqus Analysis User's Guide.
To define concrete smeared cracking:
From the menu bar in the Edit Material dialog box, select MechanicalPlasticityConcrete Smeared Cracking.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
Enter the following data in the Data table:
Comp Stress
Absolute value of compressive stress. (Units of FL–2.)
Plastic Strain
Absolute value of plastic strain. The first stress-strain point given at each value of temperature and field variable must be at zero plastic strain and will define the initial yield point for that temperature and field variable.
Temp
Temperature.
Field n
Predefined field variables.
Select Tension Stiffening from the Suboptions menu to model the postfailure behavior for direct straining across cracks. See “Defining tension stiffening for a concrete smeared cracking model” for details.
If desired, select Shear Retention from the Suboptions menu to define how shear stiffness diminishes as the concrete cracks. See “Defining shear retention for a concrete smeared cracking model” for details.
If desired, select Failure Ratios from the Suboptions menu to define the shape of the failure surface. See “Defining the shape of the failure surface for a concrete smeared cracking model” for details.
Click OK to create the material and to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
You can model postfailure behavior for direct straining across cracks with tension stiffening, which allows you to define the strain-softening behavior for cracked concrete. This behavior also allows the effects of the reinforcement interaction with concrete to be simulated in a simple manner.
You can specify tension stiffening by means of a postfailure stress-strain relation or by applying a fracture energy cracking criterion. See “Tension stiffening” in “Concrete smeared cracking,” Section 23.6.1 of the Abaqus Analysis User's Guide, for more information.
Tension stiffening information is required for the concrete smeared cracking model.
To define tension stiffening:
Create a material model as described in “Specifying a concrete smeared cracking model.”
From the Suboptions menu, select Tension Stiffening.
A Suboption Editor appears.
Click the arrow to the right of the Type field, and select a method for defining postcracking behavior:
Select Displacement to enter the displacement at which a linear loss of strength after cracking gives zero stress.
Select Strain to enter the postfailure stress-strain relationship directly.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
In the Data table, enter the data relevant to your Type choice from Step 3 (not all of the following will apply):
Disp
Displacement, 
, at which a linear loss of strength after cracking gives zero stress. (Units of L.)
sigma/sigma_c
Fraction of remaining stress to stress at cracking.
epsilon-epsilon_c
Absolute value of the direct strain minus the direct strain at cracking.
Temp
Temperature.
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
As concrete cracks, its shear stiffness is diminished. You can define this effect by specifying the reduction in the shear modulus as a function of the opening strain across the crack. You can also specify a reduced shear modulus for closed cracks. See “Cracked shear retention” in “Concrete smeared cracking,” Section 23.6.1 of the Abaqus Analysis User's Guide, for more information.
If you do not define shear retention for a concrete smeared cracking model, Abaqus/Standard automatically assumes that the shear response is unaffected by cracking (full shear retention). This assumption is often reasonable: in many cases, the overall response is not strongly dependent on the amount of shear retention.
To define shear retention:
Create a material model as described in “Specifying a concrete smeared cracking model.”
From the Suboptions menu, select Shear Retention.
A Suboption Editor appears.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
Enter the following data in the Data table:
Rho_close
The multiplying factor, 
, that defines the modulus for shearing of closed cracks as a fraction of the elastic shear modulus of the uncracked concrete. The default value is 1.0.
Eps_max
The maximum direct strain across the crack, 
. The default value is a very large number (full shear retention).
Temp
Temperature.
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
You can specify failure ratios to define the shape of the failure surface. If you do not define the shape of the failure surface, Abaqus uses the default values listed below.
To specify failure ratios:
Create a material model as described in “Specifying a concrete smeared cracking model.”
From the Suboptions menu, select Failure Ratios.
A Suboption Editor appears.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
Enter the following data in the Data table:
Ratio 1
Ratio of the ultimate biaxial compressive stress to the uniaxial compressive ultimate stress. The default value is 1.16.
Ratio 2
Absolute value of the ratio of uniaxial tensile stress at failure to the uniaxial compressive stress at failure. The default value is 0.09.
Ratio 3
Ratio of the magnitude of a principal component of plastic strain at ultimate stress in biaxial compression to the plastic strain at ultimate stress in uniaxial compression. The default value is 1.28.
Ratio 4
Ratio of the tensile principal stress value at cracking in plane stress, when the other nonzero principal stress component is at the ultimate compressive stress value, to the tensile cracking stress under uniaxial tension. The default value is 1/3.
Temp
Temperature.
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
The crushable foam model allows you to define not only crushable foams that are typically used as energy absorption structures, but also other crushable materials other than foams. See “Crushable foam plasticity models,” Section 23.3.5 of the Abaqus Analysis User's Guide, for more information.
You can use the crushable foam model to model the enhanced ability of a foam material to deform in compression due to cell wall buckling processes. This model is based on the assumption that the resulting deformation is not recoverable instantaneously and can be idealized as plastic for short duration events. See “Crushable foam plasticity models,” Section 23.3.5 of the Abaqus Analysis User's Guide, for more information.
To define a crushable foam model:
From the menu bar in the Edit Material dialog box, select MechanicalPlasticityCrushable Foam.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Click the arrow to the right of the Hardening field, and select a hardening model:
Select Volumetric to specify a model that assumes that the yield surface is controlled by the volumetric compacting plastic strain experienced by the material. Volumetric hardening is the only model available for Abaqus/Standard analyses.
Select Isotropic to specify a model that uses a yield surface that is an ellipse centered at the origin in the p–q stress plane. The yield surface evolves in a self-similar manner, and the evolution is governed by the equivalent plastic strain. This model is available only for Abaqus/Explicit analyses.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
In the Data table, enter the data relevant to your Hardening choice from Step 2 (not all of the following will apply):
Compression Yield Stress Ratio
Yield stress ratio for compression loading, 
; 
. Enter the ratio of initial yield stress in uniaxial compression to initial yield stress in hydrostatic compression.
Hydrostatic Yield Stress Ratio
Yield stress ratio for hydrostatic loading, 
; 
. Enter the ratio of yield stress in hydrostatic tension to initial yield stress in hydrostatic compression, provided as a positive value. The default value is 1.0.
Plastic Poisson's Ratio
Plastic Poisson's ratio, 
; 
.
Temp
Temperature.
Field n
Predefined field variables.
Select Foam Hardening from the Suboptions menu to define hardening data for the crushable foam model. See “Defining crushable foam hardening” for details.
If desired, select Rate Dependent from the Suboptions menu to specify strain-rate-dependent material behavior. See “Defining rate dependence for a crushable foam plasticity model” for details.
Click OK to create the material and to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
You must provide crushable foam hardening data to complete a crushable foam plasticity definition. See “Crushable foam plasticity models,” Section 23.3.5 of the Abaqus Analysis User's Guide, for more information.
To define crushable foam hardening:
Create a material model as described in “Specifying a crushable foam model.”
From the Suboptions menu, select Crushable Foam Hardening.
A Suboption Editor appears.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
Enter the following data in the Data table:
Yield Stress
Yield stress in uniaxial compression, , provided as a positive value.
Vol Plastic Strain
Absolute value of the corresponding plastic strain. (The first tabular value entered must always be zero.)
Temp
Temperature.
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
As strain rates increase, many materials show an increase in the yield stress. For many crushable foam materials this increase in yield stress becomes important when the strain rates are in the range of 0.1–1 per second and can be very important if the strain rates are in the range of 10–100 per second, as commonly occurs in high-energy dynamic events.
For more information on strain rate dependence, see “Crushable foam plasticity models,” Section 23.3.5 of the Abaqus Analysis User's Guide, and “Rate-dependent yield,” Section 23.2.3 of the Abaqus Analysis User's Guide.
To define rate dependent yield:
Create a material model as described in “Specifying a crushable foam model.”
From the Suboptions menu in the Edit Material dialog box, select Rate Dependent.
A Suboption Editor appears.
Click the arrow to the right of the Hardening field, and select a method for defining hardening dependencies:
Select Power Law to define yield stress ratios with the Cowper-Symonds overstress law.
Select Tabular to enter yield stress ratios directly in tabular form as a function of equivalent plastic strain rates.
If applicable, toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
If applicable, click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
If you selected Power Law from the list of Hardening options, enter the following data in the Data table:
Mulitiplier
Material parameter, D.
Exponent
Material parameter, n.
Temp
Temperature.
Field n
Predefined field variables.
If you selected Yield Ratio from the list of Hardening options, enter the following data in the Data table:
Yld Stress Ratio
Yield stress ratio, .
Eq Plastic Strain Rate
Equivalent plastic strain rate, (or , the absolute value of the axial plastic strain rate in uniaxial compression, for the crushable foam model).
Temp
Temperature.
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
You can define a Drucker-Prager model to model frictional materials, which are typically granular-like soils and rock and exhibit pressure-dependent yield. See “Extended Drucker-Prager models,” Section 23.3.1 of the Abaqus Analysis User's Guide, for more information.
The extended Drucker-Prager family of plasticity models describes the behavior of granular materials or polymers in which the yield behavior depends on the equivalent pressure stress. The inelastic deformation may sometimes be associated with frictional mechanisms such as sliding of particles across each other. See “Extended Drucker-Prager models,” Section 23.3.1 of the Abaqus Analysis User's Guide, for more information.
To define a Drucker-Prager plasticity model:
From the menu bar in the Edit Material dialog box, select MechanicalPlasticityDrucker Prager.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Click the arrow to the right of the Shear criterion field, and specify which yield criterion you want to define. See the following sections for more information:
If you are performing an Abaqus/Standard analysis, enter a value for the Flow potential eccentricity, .
The eccentricity is a small positive number that defines the rate at which the hyperbolic flow potential approaches its asymptote. The default is for the exponent model, and if 
, it is set to 
for the hyperbolic model to ensure associated flow. See “Extended Drucker-Prager models,” Section 23.3.1 of the Abaqus Analysis User's Guide, for more information.
If you selected Exponent Form from the list of Shear criterion options, you can toggle on Use Suboption Triaxial Test Data to request that Abaqus compute the material constants from triaxial test data at different levels of confining pressure. See “General exponent model” in “Extended Drucker-Prager models,” Section 23.3.1 of the Abaqus Analysis User's Guide, for more information.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
In the Data table, enter the data relevant to your Shear criterion choice (not all of the following will apply):
Angle of Friction
If you selected Linear from the list of Shear criterion options, enter the material angle of friction, , in the p–t plane.
If you selected Hyperbolic from the list of Shear criterion options, enter the material angle of friction, , at high confining pressure in the p–q plane.
Enter the value in degrees.
Flow Stress Ratio
The ratio of the flow stress in triaxial tension to the flow stress in triaxial compression, K. . If you leave this field blank or enter a value of 0.0 is entered, Abaqus uses a default of 1.0. If you plan to define creep behavior, set K to 1.0.
Dilation Angle
If you selected Linear from the list of Shear criterion options, enter the dilation angle, , in the p–t plane.
If you selected Hyperbolic or Exponent Form from the list of Shear criterion options, enter the dilation angle, , at high confining pressure in the p–q plane.
Enter the value in degrees.
Init Tension
Initial hydrostatic tension strength, 
. (Units of FL–2.)
a
Material constant a.
b
Exponent b. To ensure a convex yield surface, 
.
Select Drucker Prager Hardening from the Suboptions menu to specify hardening data for the Drucker-Prager model. See “Defining Drucker-Prager hardening” for details.
If desired, select Drucker Prager Creep from the Suboptions menu to specify creep data for the Drucker-Prager model. This option is valid only if you have selected Linear from the list of Shear criterion options and are performing an Abaqus/Standard analysis. See “Defining Drucker-Prager creep” for details.
If you toggled on Use Suboption Triaxial Test Data in Step 4, select Triaxial Test Data from the Suboptions menu to enter the triaxial test data. See “Specifying triaxial test data for a Drucker-Prager material model” for details.
Click OK to create the material and to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
Use the Suboption Editor to specify hardening data for a Drucker-Prager model. For more information on Drucker-Prager hardening, see “Hardening and rate dependence” in “Extended Drucker-Prager models,” Section 23.3.1 of the Abaqus Analysis User's Guide.
To define Drucker-Prager hardening:
Create a material model as described in “Defining a Drucker-Prager model.”
From the Suboptions menu in the Edit Material dialog box, select Drucker Prager Hardening.
A Suboption Editor appears.
Select the Hardening behavior type of your choice.
The evolution of the yield surface with plastic deformation is described in terms of the equivalent stress 
, which you can choose to be either the uniaxial Compression yield stress, the uniaxial Tension yield stress, or the Shear (cohesion) yield stress
Toggle on Use strain-rate-dependent data if you want enter data showing yield stress values versus equivalent plastic strain at different equivalent plastic strain rates.
A Rate column appears in the Data table.
Alternatively, if you want to define strain rate dependence using yield stress ratios, you must select Rate Dependent from the Suboptions menu in the Edit Material dialog box. See “Defining rate-dependent yield with yield stress ratios” for details. For background information on rate dependence, see “Rate-dependent yield,” Section 23.2.3 of the Abaqus Analysis User's Guide.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
Enter the following data in the Data table:
Yield Stress
Yield stress.
Abs Plastic Strain
Absolute value of the corresponding plastic strain. (The first tabular value entered must always be zero.)
Rate
Equivalent plastic strain rate, 
, for which this hardening curve applies.
Temp
Temperature.
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
You can define classical “creep” behavior of materials that exhibit plasticity according to the extended Drucker-Prager models in Abaqus/Standard analyses. The creep behavior in such materials is intimately tied to the plasticity behavior (through the definitions of creep flow potentials and definitions of test data), so you must include both Drucker-Prager plasticity and Drucker-Prager hardening data in the material definition.
The creep data that you enter must be consistent with the Hardening behavior type that you select when defining Drucker-Prager hardening (see “Defining Drucker-Prager hardening” for details).
For more information, see “Creep models for the linear Drucker-Prager model” in “Extended Drucker-Prager models,” Section 23.3.1 of the Abaqus Analysis User's Guide.
To define Drucker-Prager creep:
Create a material model as described in “Defining a Drucker-Prager model.”
From the Suboptions menu in the Edit Material dialog box, select Drucker Prager Creep.
A Suboption Editor appears.
Click the arrow to the right of the Law field, and select the creep law option of your choice:
Select Strain to choose a strain hardening power law.
Select Time to choose a time hardening power law
Select SinghM to choose a Singh-Mitchell type law.
Select User to specify the creep law with user subroutine CREEP.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
If you selected either the Strain or the Time creep law option, enter the following data in the Data table:
A, n, and m
Creep material parameters.
Temp
Temperature.
Field n
Predefined field variables.
If you selected the SinghM creep law option, enter the following data in the Data table:
A, alpha, m, and t1
Creep material parameters A, , , and m.
Temp
Temperature.
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
Abaqus can use triaxial test data to calibrate the material parameters that define the Exponent Form of Drucker-Prager plasticity. See “General exponent model” in “Extended Drucker-Prager models,” Section 23.3.1 of the Abaqus Analysis User's Guide, for more information.
To enter triaxial test data:
Create a material model as described in “Defining a Drucker-Prager model.”
From the Suboptions menu in the Edit Material dialog box, select Triaxial Test Data.
A Suboption Editor appears.
Enter values for Material constant a, Material constant b, and Material constant pt if they are known and held fixed at the input value. Alternatively, you can leave one or more of the fields blank if you want Abaqus to calibrate the values from the triaxial test data.
Enter the following data in the Data table:
Confining Stress
Sign and magnitude of the confining stress, 
.
Loading Dirn Stress
Sign and magnitude of the stress in the loading direction, 
.
Click OK to return to the Edit Material dialog box.
You can use the Mohr-Coulomb plasticity model for geotechnical engineering design applications. The model uses the classical Mohr-Coloumb yield criterion: a straight line in the meridional plane and an irregular hexagonal section in the deviatoric plane. However, the Abaqus Mohr-Coulomb model has a completely smooth flow potential instead of the classical hexagonal pyramid: the flow potential is a hyperbola in the meridional plane, and it uses the smooth deviatoric section proposed by Menétrey and Willam. See “Mohr-Coulomb plasticity,” Section 23.3.3 of the Abaqus Analysis User's Guide, for more information.
To define Mohr-Coulomb plasticity:
From the menu bar in the Edit Material dialog box, select MechanicalPlasticityMohr Coulomb Plasticity.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Click the Plasticity tab, if necessary, to display the Plasticity tabbed page.
Choose how you want to define Deviatoric eccentricity, e:
Select Calulated default to allow Abaqus to calculate the deviatoric eccentricity as 
, where 
is the Mohr-Coulomb Friction Angle that you specify in the Data table.
Select Specify, and enter a value for deviatoric eccentricity in the field provided. The range of values e can have is 
.
Enter a value for Meridional eccentricity, .
The meridional eccentricity is a small positive number that defines the rate at which the flow potential approaches its asymptote.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
Enter the following data in the Data table:
Friction Angle
Friction angle, , at high confining pressure in the p–
plane. Enter the value in degrees.
Dilation Angle
Dilation angle, , at high confining pressure in the p–
plane. Enter the value in degrees.
Temp
Temperature.
Field n
Predefined field variables.
Click the Cohesion tab to display the Cohesion tabbed page.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
Enter the following data in the Data table:
Cohesion Yield Stress
Cohesion yield stress.
Abs Plastic Strain
Absolute value of the corresponding plastic strain. (The first tabular value entered must always be zero.)
Temp
Temperature.
Field n
Predefined field variables.
If desired, toggle on Specify tension cutoff and click the Tension Cutoff tab to specify tension cutoff stress data to limit the load carrying capacity of the material model near the tensile region.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
Enter the following data in the Data table:
Tension Cutoff Stress
Yield stress in uniaxial tension, .
Tensile Plastic Strain
Corresponding plastic strain. (The first tabular value entered must always be zero.)
Temp
Temperature.
Field n
Predefined field variables.
Click OK to create the material and to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
You can use the porous metal plasticity model for materials with a dilute concentration of voids in which the relative density is greater than 0.9. See “Porous metal plasticity,” Section 23.2.9 of the Abaqus Analysis User's Guide, for more information.
The porous metal plasticity model describes materials that exhibit damage in the form of void initiation and growth. You can also use this model for some powder metal process simulations at high relative densities (relative density is defined as the ratio of the volume of solid material to the total volume of the material). The model is based on Gurson's porous metal plasticity theory with void nucleation and is intended for use with materials that have a relative density that is greater than 0.9. The model is adequate for relatively monotonic loading.
See “Porous metal plasticity,” Section 23.2.9 of the Abaqus Analysis User's Guide, for more information.
Defining porous metal plasticity:
From the menu bar in the Edit Material dialog box, select MechanicalPlasticityPorous Metal Plasticity.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Enter a value for the initial Relative density of the material.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
Enter the following data in the Data table:
q1, q2, and q3
Material parameters 
, 
, 
.
For typical metals the ranges of the parameters reported in the literature are = 1.0 to 1.5, = 1.0, and = 
= 1.0 to 2.25 (see “Necking of a round tensile bar,” Section 1.1.9 of the Abaqus Benchmarks Guide). The original Gurson model is recovered when = = = 1.0.
Temp
Temperature.
Field n
Predefined field variables.
If desired, select Porous Failure Criteria from the Suboption menu to specify material failure criteria for an Abaqus/Explicit analysis. See “Defining porous material failure criteria” for details.
If desired, select Void Nucleation from the Suboption menu to define the nucleation of voids in the porous material. See “Defining void nucleation in a porous material” for details.
Click OK to create the material and to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
You use the Suboption Editor to define failure in a porous metal plasticity model. See “Failure criteria in Abaqus/Explicit” in “Porous metal plasticity,” Section 23.2.9 of the Abaqus Analysis User's Guide, for more information.
To specify porous metal failure criteria:
Create a material model as described in “Defining a porous metal plasticity model.”
From the Suboptions menu in the Edit Material dialog box, select Porous Failure Criteria.
A Suboption Editor appears.
Enter a value for the Total volume void fraction at total failure, 
. The default is 1.
Enter a value for the Critical void volume fraction (threshold of rapid loss of stress carrying capacity), 
. The default is 
.
Click OK to return to the Edit Material dialog box.
You use the Suboption Editor to define the nucleation of voids in a porous metal plasticity model. See “Void growth and nucleation” in “Porous metal plasticity,” Section 23.2.9 of the Abaqus Analysis User's Guide, for more information.
To define void nucleation:
Create a material model as described in “Defining a porous metal plasticity model.”
From the Suboptions menu in the Edit Material dialog box, select Void Nucleation.
A Suboption Editor appears.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
Enter the following data in the Data table:
Mean
Mean value of the nucleation-strain normal distribution, 
.
Standard Deviation
Standard deviation of the nucleation-strain normal distribution, 
.
Volume Fraction
Volume fraction of nucleating voids, 
.
Temp
Temperature.
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
If you are performing an Abaqus/Standard analysis, you can define classical deviatoric metal creep behavior either by specifying user subroutine CREEP or by providing parameters for some simple creep laws. See “Rate-dependent plasticity: creep and swelling,” Section 23.2.4 of the Abaqus Analysis User's Guide, for more information.
To define creep:
From the menu bar in the Edit Material dialog box, select MechanicalPlasticityCreep.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Click the arrow to the right of the Law field, and select the creep law of your choice. See “Creep behavior” in “Rate-dependent plasticity: creep and swelling,” Section 23.2.4 of the Abaqus Analysis User's Guide, for more information.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
If you selected the Strain-Hardening or Time-Hardening creep law, enter the following data in the Data table:
Power Law Multiplier
Power law multiplier, A. (Units of F
L
T
.)
Eq Stress Order
Equivalent deviatoric stress order, n.
Time Order
Total time order, m, for the Time-Hardening creep law, or strain order, m, for the Strain-Hardening creep law.
Temp
Temperature.
Field n
Predefined field variables.
If you selected the Hyperbolic-Sine creep law, enter the following data in the Data table:
Power Law Multiplier
Power law multiplier, A. (Units of T–1.)
Hyperb Law Multiplier
Hyperbolic sine law multiplier, B. (Units of F–1L2.)
Eq Stress Order
Equivalent stress order, n
Activation Energy
Activation energy, 
. (Units of JM–1
Univeral Gas Const
Universal gas constant, R. (Units of JM–1–1.)
Temp
Temperature.
Field n
Predefined field variables.
If desired, select Ornl from the Suboptions menu to implement the creep rules specified by the Oak Ridge National Laboratory constitutive model. See “Using the Oak Ridge National Laboratory (ORNL) constitutive model in plasticity and creep calculations” for more information.
If desired, select Potential from the Suboptions menu to specify anisotropic creep behavior. See “Defining anisotropic yield and creep” for more information.
Click OK to create the material and to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
User subroutine CREEP (“CREEP,” Section 1.1.1 of the Abaqus User Subroutines Reference Guide) provides a very general capability for implementing viscoplastic models such as creep and swelling models. However, you can also enter swelling data in tabular form. See “Volumetric swelling behavior” in “Rate-dependent plasticity: creep and swelling,” Section 23.2.4 of the Abaqus Analysis User's Guide, for more information.
As with the creep laws, volumetric swelling laws are usually complex and are most conveniently specified in user subroutine CREEP. However, you can also enter tabular swelling data in the Edit Material dialog box. See “Volumetric swelling behavior” in “Rate-dependent plasticity: creep and swelling,” Section 23.2.4 of the Abaqus Analysis User's Guide, for more information.
To define swelling:
From the menu bar in the Edit Material dialog box, select MechanicalPlasticitySwelling.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Click the arrow to the right of the Law field, and select an option for specifying swelling data:
Select Input to enter tabular data in the Edit Material dialog box.
Select User-defined to define the swelling behavior in user subroutine CREEP
If you selected Input in Step 2, toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
If you selected Input in Step 2, click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
If you selected Input in Step 2, enter the following data in the Data table:
Strain Rate
Volumetric swelling strain rate.
Temp
Temperature.
Field n
Predefined field variables.
If desired, select Ratios from the Suboptions menu to define anisotropic swelling. See “Defining anisotropic swelling” for details.
Click OK to create the material and to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
You can specify ratios in the Suboptions Editor to define the swelling rate in each material direction. See “Volumetric swelling behavior” in “Rate-dependent plasticity: creep and swelling,” Section 23.2.4 of the Abaqus Analysis User's Guide, for more information.
To define anisotropic swelling:
Create a material model as described in “Defining a volumetric swelling model.”
From the Suboptions menu in the Edit Material dialog box, select Ratios.
A Suboption Editor appears.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
Enter the following data in the Data table:
r11, r22, and r33
Anisotropic swelling ratios, 
, 
, and 
.
Temp
Temperature.
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
The two-layer viscoplasticity model in Abaqus/Standard is useful for modeling materials in which significant time-dependent behavior as well as plasticity is observed. For metals this typically occurs at elevated temperatures. This model consists of three parts: elastic, plastic, and viscous. You can define the viscous behavior of the material by selecting a creep law and entering viscosity parameters. See “Two-layer viscoplasticity,” Section 23.2.11 of the Abaqus Analysis User's Guide, for more information.
To define viscosity for a two-layer viscoplasticity model:
From the menu bar in the Edit Material dialog box, select MechanicalPlasticityViscous.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Click the arrow to the right of the Law field, and select the creep law of your choice:
Select Strain to choose a strain-hardening power law.
Select Time to choose a time-hardening power law.
Select User to define the creep law with user subroutine CREEP.
Toggle on Use temperature-dependent data to define data that depend on temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the data depend.
If you selected the Strain-Hardening or Time-Hardening creep law, enter the following data in the Data table:
A
Power law multiplier, A. (Units of FLT.)
n
Equivalent deviatoric stress order, n.
m
Total time or equivalent creep strain order, m.
f
The fraction, f, that defines the ratio of the elastic modulus of the elastic-viscous network to the total (instantaneous) modulus.
Temp
Temperature.
Field n
Predefined field variables.
If you are defining the creep law with user subroutine CREEP, enter the following in the Data table:
f
The fraction, f, that defines the ratio of the elastic modulus of the elastic-viscous network to the total (instantaneous) modulus.
Temp
Temperature.
Field n
Predefined field variables.
If desired, select Potential from the Suboptions menu to define anisotropic viscosity. See “Defining anisotropic yield and creep” for details.
Click OK to create the material and to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).