You use the Edit Material dialog box to create an elastic material and to specify its elastic material properties. You can create the following elastic material models:
Elastic; see “Creating a linear elastic material model”
Isotropic Hyperelastic; see “Creating an isotropic hyperelastic material model”
Anisotropic Hyperelastic; see “Creating an anisotropic hyperelastic material model”
Hyperfoam; see “Creating a hyperfoam material model”
Low-Density Foam; see “Creating a low-density foam material model”
Hypoelastic; see “Creating a hypoelastic material model”
Porous Elastic; see “Creating a porous elastic material model”
Viscoelastic; see “Creating a viscoelastic material model”
Linear elasticity is the simplest form of elasticity available in Abaqus. The linear elastic model can define isotropic, orthotropic, or anisotropic material behavior and is valid for small elastic strains. See “Specifying elastic material properties” for details on how to define a linear elastic material model.
Failure theories are provided for use with linear elasticity. They can be used to obtain postprocessed output requests. The following sections describe how to specify these failure models:
A linear elastic material model is valid for small elastic strains (normally less than 5%); can be isotropic, orthotropic, or fully anisotropic; and can have properties that depend on temperature and/or other field variables. For more information, see “Linear elastic behavior,” Section 22.2.1 of the Abaqus Analysis User's Guide.
To specify elastic material properties:
From the menu bar in the Edit Material dialog box, select Mechanical
ElasticityElastic.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
From the Type field, choose the type of data you will supply to specify the elastic material properties.
Choose Isotropic to specify isotropic elastic properties, as described in “Defining isotropic elasticity” in “Linear elastic behavior,” Section 22.2.1 of the Abaqus Analysis User's Guide.
Choose Engineering Constants to specify orthotropic elastic properties by giving the engineering constants, as described in “Defining orthotropic elasticity by specifying the engineering constants” in “Linear elastic behavior,” Section 22.2.1 of the Abaqus Analysis User's Guide.
Choose Lamina to specify orthotropic elastic properties in plane stress, as described in “Defining orthotropic elasticity in plane stress” in “Linear elastic behavior,” Section 22.2.1 of the Abaqus Analysis User's Guide.
Choose Orthotropic to specify orthotropic elastic properties directly, as described in “Defining orthotropic elasticity by specifying the terms in the elastic stiffness matrix” in “Linear elastic behavior,” Section 22.2.1 of the Abaqus Analysis User's Guide.
Choose Anisotropic to specify anisotropic elastic properties, as described in “Defining fully anisotropic elasticity” in “Linear elastic behavior,” Section 22.2.1 of the Abaqus Analysis User's Guide.
Choose Traction to specify orthotropic elastic properties for warping elements, as described in “Defining orthotropic elasticity for warping elements” in “Linear elastic behavior,” Section 22.2.1 of the Abaqus Analysis User's Guide, or to define uncoupled elastic properties for cohesive elements, as described in “Defining elasticity in terms of tractions and separations for cohesive elements” in “Linear elastic behavior,” Section 22.2.1 of the Abaqus Analysis User's Guide.
Choose Coupled Traction to specify coupled elastic properties for cohesive elements, as described in “Defining elasticity in terms of tractions and separations for cohesive elements” in “Linear elastic behavior,” Section 22.2.1 of the Abaqus Analysis User's Guide.
Choose Shear to specify a linear isotropic deviatoric material model. For more information, see “Deviatoric behavior” in “Equation of state,” Section 25.2.1 of the Abaqus Analysis User's Guide.
To define behavior data that depend on temperature, toggle on Use temperature-dependent data.
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.
Field variable columns appear in the Data table.
If you are defining the elastic behavior of a viscoelastic material, click the arrow to the right of the Moduli time scale (for viscoelasticity) field to specify either long-term or instantaneous elastic response.
Toggle on No compression if you want to modify the elastic material response such that compressive stress cannot be generated. For details, see “No compression or no tension,” Section 22.2.2 of the Abaqus Analysis User's Guide.
Toggle on No tension if you want to modify the elastic material response such that tensile stress cannot be generated. For details, see “No compression or no tension,” Section 22.2.2 of the Abaqus Analysis User's Guide.
Enter the material properties in the Data table.
For Isotropic data, enter the Young's modulus, E, and Poisson's ratio, 
.
For Engineering Constants data, enter the generalized Young's moduli in the principal directions, 
, 
, 
; the Poisson's ratios in the principal directions, 
, 
, 
; and the shear moduli in the principal directions, 
, 
, 
.
For Lamina data, enter the Young's moduli, , ; the Poisson's ratio, ; and the shear moduli, , , . The and shear moduli are needed to define transverse shear behavior in shells.
For Orthotropic data, enter the 9 elastic stiffness parameters: 
, 
, etc. (units of FL–2).
For Anisotropic data, enter the 21 elastic stiffness parameters: , , etc. (units of FL–2).
For Traction data, your entries depend on the element type that you are modeling.
For solid cross-section Timoshenko beam elements modeled with warping elements, enter the Young's modulus, 
, and the shear moduli in the material directions, 
and 
.
For cohesive elements with uncoupled traction, enter the elastic modulus in the normal direction and the two local shear directions, 
, 
, and 
.
For Coupled Traction data, enter the six elastic moduli: , , , 
, 
, and 
.
For Shear data, enter the Shear Modulus.
To define the plane stress orthotropic failure measures for the material, if desired, click Suboptions. For details, see the following sections:
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 define the stress limits for stress-based failure measures for an elastic material model. For more information, see “Plane stress orthotropic failure measures,” Section 22.2.3 of the Abaqus Analysis User's Guide.
To define stress-based failure measures for an elastic model:
Create a linear elastic material model as described in “Specifying elastic material properties.”
From the Suboptions menu in the Edit Material dialog box, select Fail Stress.
The Suboption Editor appears.
To define behavior data that depend on temperature, toggle on Use temperature-dependent data.
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.
Field variable columns appear in the Data table.
In the Data table, enter the stress limits:
Ten Stress Fiber Dir
Tensile stress limit in the fiber direction, 
.
Com Stress Fiber Dir
Compressive stress limit in the fiber direction, 
.
Ten Stress Transv Dir
Tensile stress limit in the transverse direction, 
.
Com Stress Transv Dir
Compressive stress limit in the transverse direction, 
.
Shear Strength
Shear strength in the X–Y plane, S.
Cross-prod Term Coeff
Cross product term coefficient, 
(
). This value is used only for the Tsai-Wu theory and is ignored if 
is provided. The default is zero.
Stress Limit
Biaxial stress limit, . This value is used only for the Tsai-Wu theory. If this entry is nonzero, is ignored.
Click OK to return to the Edit Material dialog box.
Use the Suboption Editor to define the strain limits for strain-based failure measures for an elastic material model. For more information, see “Plane stress orthotropic failure measures,” Section 22.2.3 of the Abaqus Analysis User's Guide.
To define strain-based failure measures:
Create a linear elastic material model as described in “Specifying elastic material properties.”
From the Suboptions menu in the Edit Material dialog box, select Fail Strain.
To define behavior data that depend on temperature, toggle on Use temperature-dependent data.
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.
Field variable columns appear in the Data table.
In the Data table, enter the strain limits:
Ten Strain Fiber Dir
Tensile strain limit in the fiber direction, 
.
Com Strain Fiber Dir
Compressive strain limit in the fiber direction, 
.
Ten Strain Transv Dir
Tensile strain limit in the transverse direction, 
.
Com Strain Transv Dir
Compressive strain limit in the transverse direction, 
.
Shear Strain
Shear strain limit in the X–Y plane, 
.
Click OK to return to the Edit Material dialog box.
The isotropic hyperelastic model describes the behavior of nearly incompressible materials that exhibit instantaneous elastic response up to large strains. For more information, see “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
Isotropic hyperelastic materials are described in terms of a “strain energy potential,” which defines the strain energy stored in the material per unit of reference volume (volume in the initial configuration) as a function of the strain at that point in the material. Several forms of strain energy potentials are available in Abaqus to model approximately incompressible isotropic elastomers. For more information on hyperelastic materials, see “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
When you define a isotropic hyperelastic material, you have the option of either specifying material parameters directly or allowing Abaqus to calculate them from test data that you provide. For detailed instructions, see the following sections:
You can provide the parameters of the hyperelastic strain energy potentials directly as functions of temperature.
To specify an isotropic hyperelastic material by specifying the material constants directly:
From the menu bar in the Edit Material dialog box, select MechanicalElasticityHyperelastic.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Choose Isotropic as the material type.
Click the arrow to the right of the Strain energy potential field, and select the strain energy potential of your choice.
Arruda-Boyce: The Arruda-Boyce model is also known as the eight-chain model. For more information, see “Arruda-Boyce form” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
Marlow: For more information, see “Marlow form” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
Mooney-Rivlin: The Mooney-Rivlin model is equivalent to using the polynomial model with N=1. For more information, see “ Mooney-Rivlin form” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
Neo Hooke: The Neo Hookean model is equivalent to using the reduced polynomial model with N=1. For more information, see “Neo-Hookean form” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
Ogden: For more information, see “Ogden form” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
Polynomial: For more information, see “Polynomial form” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
Reduced Polynomial: The reduced polynomial model is equivalent to using the polynomial model with 
for 
. For more information, see “Reduced polynomial form” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
User-defined: You can define the derivatives of the strain energy potential with respect to the strain invariants in user subroutine UHYPER. This method is valid only for Abaqus/Standard analyses. For more information, see “User subroutine specification in Abaqus/Standard” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
Van der Waals: The Van der Waals model is also known as the Kilian model. For more information, see “Van der Waals form” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
Yeoh: The Yeoh model is equivalent to using the reduced polynomial model with N=3. For more information, see “Yeoh form” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
Unknown: If you define an isotropic hyperelastic material using experimental data, you also have the option of temporarily leaving the particular strain energy potential unspecified. You can use the Evaluate option to identify the optimal strain energy potential for the material data and display the material editor again to complete the material definition; see “Evaluating hyperelastic and viscoelastic material behavior,” Section 12.4.7, for more information.
Select Coefficients as the Input source. This Input Source option is invalid for the Marlow model or for an unknown strain energy potential.
If you are defining the hyperelastic behavior of a viscoelastic material, click the arrow to the right of the Moduli time scale (for viscoelasticity) field to specify either long-term or instantaneous elastic response.
If you selected User-defined as the strain energy potential, perform the following steps:
If you selected Ogden, Polynomial, or Reduced Polynomial as the strain energy potential, click the arrows to the left of the Strain energy potential order field to select a value.
To define behavior data that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the Data table.
Enter the material properties in the Data table corresponding to the chosen strain energy potential.
Arruda-Boyce
Enter 
, 
, and D.
Mooney-Rivlin
Enter 
, 
, and 
.
Neo Hooke
Enter and .
Ogden
Enter 
, 
, and 
, where i goes from 1 to N and N is the value specified for the Strain energy potential order.
Polynomial
Enter 
, where 
goes from 1 to N, and , where i goes from 1 to N, and N is the value specified for the Strain energy potential order.
Reduced Polynomial
Enter 
and , where i goes from 1 to N and N is the value specified for the Strain energy potential order.
Van der Waals
Enter , , a, 
, and D.
Yeoh
Enter , 
, 
, , 
, and 
.
If desired, select Hysteresis from the Suboptions menu to define hysteretic behavior. See “Defining hysteretic behavior for an isotropic hyperelastic 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).
Abaqus can calculate material parameters from test data that you enter in the Test Data Editor.
To specify an isotropic hyperelastic material by providing test data:
From the menu bar in the Edit Material dialog box, select MechanicalElasticityHyperelastic.
(For information on displaying the Edit Material dialog box, see Creating and editing materials, Section 12.7. .)
Choose Isotropic as the material type.
Click the arrow to the right of the Strain energy potential field, and select the strain energy potential of your choice.
Arruda-Boyce: The Arruda-Boyce model is also known as the eight-chain model. For more information, see “Arruda-Boyce form” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
Marlow: For more information, see “Marlow form” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
Mooney-Rivlin: The Mooney-Rivlin model is equivalent to using the polynomial model with N=1. For more information, see “ Mooney-Rivlin form” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
Neo Hooke: The Neo Hookean model is equivalent to using the reduced polynomial model with N=1. For more information, see “Neo-Hookean form” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
Ogden: For more information, see “Ogden form” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
Polynomial: For more information, see “Polynomial form” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
Reduced Polynomial: The reduced polynomial model is equivalent to using the polynomial model with for . For more information, see “Reduced polynomial form” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
User-defined: You can define the derivatives of the strain energy potential with respect to the strain invariants in user subroutine UHYPER. This method is valid only for Abaqus/Standard analyses. For more information, see “User subroutine specification in Abaqus/Standard” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
Van der Waals: The Van der Waals model is also known as the Kilian model. For more information, see “Van der Waals form” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
Yeoh: The Yeoh model is equivalent to using the reduced polynomial model with N=3. For more information, see “Yeoh form” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
Unknown: If you define an isotropic hyperelastic material using experimental data, you also have the option of temporarily leaving the particular strain energy potential unspecified. You can use the Evaluate option to identify the optimal strain energy potential for the material data and then display the material editor again to complete the material definition; see “Evaluating hyperelastic and viscoelastic material behavior,” Section 12.4.7, for more information.
Select Test data as the Input source to indicate that the material constants are to be computed from data taken from simple tests on a material specimen.
If you are defining the hyperelastic behavior of a viscoelastic material, click the arrow to the right of the Moduli time scale (for viscoelasticity) field to specify either long-term or instantaneous elastic response.
If you selected Marlow as the strain energy potential, select the Data to define deviatoric response and the Data to define volumetric response options of your choice.
The deviatoric response is defined by the Uniaxial, Biaxial, or Planar test data specified as described in Step 8.
The volumetric response is defined by one of the following methods:
Ignore test data: Abaqus/Standard assumes fully incompressible behavior, while Abaqus/Explicit assumes compressibility corresponding to a Poisson's ratio of 0.475.
Volumetric test data: The volumetric test data are specified directly, as described in Step 8.
Poisson's ratio: Specify a value for the Poisson's ratio of the isotropic hyperelastic material.
Lateral nominal strain: Lateral nominal strains are specified as part of the uniaxial, biaxial, or planar test data, as described in Step 8.
If you selected Ogden, Polynomial, or Reduced Polynomial as the strain energy potential, click the arrows to the left of the Strain energy potential order field to select a value.
If you selected Van der Waals as the strain energy potential, choose the method for specifying Beta:
Select Fitted value to determine the value of from a nonlinear least-squares fit of the test data.
Select Specify, and enter a value to specify directly. Allowable values are 
. It is recommended to set =0 if only one type of test data is available.
You can specify the experimental stress-strain data for as many as four simple tests: uniaxial, equibiaxial, planar, and, if the material is compressible, a volumetric compression test. Use the Test Data menu to specify the experimental data. For details, see the following sections:
“Specifying uniaxial test data for an isotropic hyperelastic material model”
“Specifying biaxial test data for an isotropic hyperelastic material model”
“Specifying planar test data for an isotropic hyperelastic material model”
“Specifying volumetric test data for an isotropic hyperelastic material model”
If desired, select Hysteresis from the Suboptions menu to define hysteretic behavior. See “Defining hysteretic behavior for an isotropic hyperelastic 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 Test Data Editor to specify uniaxial test data from which Abaqus can calibrate hyperelastic material coefficients. For more information, see “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
To specify uniaxial test data:
Create an isotropic hyperelastic material model as described in “Providing test data to define an isotropic hyperelastic material.”
From the Test Data menu in the Edit Material dialog box, select Uniaxial Test Data.
A Test Data Editor appears.
Toggle on Apply smoothing if you want Abaqus to apply a smoothing filter to the stress-strain data. This option is particularly recommended if you are using the Marlow model.
If you have requested data smoothing, click the arrows to the right of the Apply smoothing field to specify the number of data points to the right and left of each data point within which Abaqus will fit a least-squares polynomial.
If you are defining a Marlow model, you can select the following options:
To include lateral nominal strain data, toggle on Include lateral nominal strain.
A column labeled Lateral Nominal Strain appears in the Data table.
To define behavior data that depend on temperature, toggle on Use temperature-dependent data.
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.
Field variable columns appear in the Data table.
In the Data table, enter the test data:
Nominal Stress
Nominal stress, 
.
Nominal Strain
Nominal strain, 
.
Lateral Nominal Strain
Nominal lateral strain, 
.
Temp
Temperature, 
.
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
Use the Test Data Editor to specify biaxial test data from which Abaqus can calibrate hyperelastic material coefficients. For more information, see “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
To specify biaxial test data:
Create an isotropic hyperelastic material model as described in “Providing test data to define an isotropic hyperelastic material.”
From the Test Data menu in the Edit Material dialog box, select Biaxial Test Data.
A Test Data Editor appears.
Toggle on Apply smoothing if you want Abaqus to apply a smoothing filter to the stress-strain data. This option is particularly recommended if you are using a Marlow model.
If you have requested data smoothing, click the arrows to the right of the Apply smoothing field to specify the number of data points to the right and left of each data point within which Abaqus will fit a least-squares polynomial.
If you are defining a Marlow model, you can select the following options:
To include lateral nominal strain data, toggle on Include lateral nominal strain.
A column labeled Lateral Nominal Strain appears in the Data table.
To define behavior data that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the Data table.
To define behavior data that depend on field variables, click the arrow to the right of the Number of field variables field to increase or decrease the number of field variables.
Field variable columns appear in the Data table.
In the Data table, enter the test data:
Nominal Stress
Nominal stress, 
.
Nominal Strain
Nominal strain, 
.
Lateral Nominal Strain
Nominal lateral strain, 
.
Temp
Temperature, .
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
Use the Test Data Editor to specify planar test data from which Abaqus can calibrate hyperelastic material coefficients. For more information, see “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
To specify planar test data:
Create an isotropic hyperelastic material model as described in “Providing test data to define an isotropic hyperelastic material.”
From the Test Data menu in the Edit Material dialog box, select Planar Test Data.
A Test Data Editor appears.
Toggle on Apply smoothing if you want Abaqus to apply a smoothing filter to the stress-strain data. This option is particularly recommended if you are using a Marlow model.
If you have requested data smoothing, click the arrows to the right of the Apply smoothing field to specify the number of data points to the right and left of each data point within which Abaqus will fit a least-squares polynomial.
If you are defining a Marlow model, you can select the following options:
To include lateral nominal strain data, toggle on Include lateral nominal strain.
A column labeled Lateral Nominal Strain appears in the Data table.
To define behavior data that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the Data table.
To define behavior data that depend on field variables, click the arrow to the right of the Number of field variables field to increase or decrease the number of field variables.
Field variable columns appear in the Data table.
In the Data table, enter the test data:
Nominal Stress
Nominal stress, 
.
Nominal Strain
Nominal strain, 
.
Lateral Nominal Strain
Nominal lateral strain, .
Temp
Temperature, .
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
Use the Test Data Editor to specify volumetric test data from which Abaqus can calibrate hyperelastic material coefficients. For more information, see “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
To specify volumetric test data:
Create an isotropic hyperelastic material model as described in “Providing test data to define an isotropic hyperelastic material.”
From the Test Data menu in the Edit Material dialog box, select Volumetric Test Data.
A Test Data Editor appears.
Toggle on Apply smoothing if you want Abaqus to apply a smoothing filter to the stress-strain data. This option is particularly recommended if you are using a Marlow model.
If you have requested data smoothing, click the arrows to the right of the Apply smoothing field to specify the number of data points to the right and left of each data point within which Abaqus will fit a least-squares polynomial.
If you are defining a Marlow model, you can select the following options:
To define behavior data that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the Data table.
To define behavior data that depend on field variables, click the arrow to the right of the Number of field variables field to increase or decrease the number of field variables.
Field variable columns appear in the Data table.
In the Data table, enter the test data:
Pressure
Total pressure stress, p.
Volume Ratio
Volume ratio (current volume/original volume), J.
Temp
Temperature, .
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
Use the Suboption Editor to define the strain-rate-dependent response of an isotropic hyperelastic material that exhibits pronounced hysteresis under cyclic loading. For more information, see “Hysteresis in elastomers,” Section 22.8.1 of the Abaqus Analysis User's Guide.
To define hysteretic material behavior:
Create an isotropic hyperelastic material model as described in “Entering material parameters to define an isotropic hyperelastic material” or “Providing test data to define an isotropic hyperelastic material.”
From the Suboptions menu in the Edit Material dialog box, select Hysteresis.
The Suboption Editor appears.
In the Data table of the Suboption Editor, enter the creep behavior data:
Stress Scaling Factor
Stress scaling factor, S.
Creep Parameter
Creep parameter, A.
Eff Stress Exponent
Effective stress exponent, m.
Creep Strain Exponent
Creep strain exponent, 
.
Click OK to return to the Edit Material dialog box.
The anisotropic hyperelastic model provides a modeling capability for materials that exhibit highly anisotropic and nonlinear elastic behavior, such as biomedical soft tissues and fiber-reinforced elastomers. For more information, see “Anisotropic hyperelastic behavior,” Section 22.5.3 of the Abaqus Analysis User's Guide.
In Abaqus/CAE the local direction vectors of the material are orthogonal and align with the axes of the assigned material orientation. The best practice is to assign the orientation using discrete orientations in Abaqus/CAE. For information about defining discrete orientations, see “Using discrete orientations for material orientations and composite layup orientations,” Section 12.16.
To specify an anisotropic hyperelastic material by specifying the material constants:
From the menu bar in the Edit Material dialog box, select MechanicalElasticityHyperelastic.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Choose Anisotropic as the material type.
Click the arrow to the right of the Strain energy potential field, and select the strain energy potential of your choice.
Fung-Anisotropic: For the fully anisotropic strain-based Fung model, you must specify 21 independent components 
. For more information, see “Generalized Fung form” in “Anisotropic hyperelastic behavior,” Section 22.5.3 of the Abaqus Analysis User's Guide.
Fung-Orthotropic: For the orthotropic strain-based Fung model, you must specify 9 independent components . For more information, see “Generalized Fung form” in “Anisotropic hyperelastic behavior,” Section 22.5.3 of the Abaqus Analysis User's Guide.
Holzapfel: This form of invariant-based strain energy potential is used for modeling arterial layers with distributed collagen fiber orientations. For more information, see “Holzapfel-Gasser-Ogden form” in “Anisotropic hyperelastic behavior,” Section 22.5.3 of the Abaqus Analysis User's Guide.
User: You can use a user subroutine to define the form of a strain-based or invariant-based strain energy potential directly. For more information, see “User-defined form: strain-based” in “Anisotropic hyperelastic behavior,” Section 22.5.3 of the Abaqus Analysis User's Guide, and “User-defined form: invariant-based” in “Anisotropic hyperelastic behavior,” Section 22.5.3 of the Abaqus Analysis User's Guide.
To define material parameters 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.
Field variable columns appear in the data table.
For the Fung-Anisotropic, Fung-Orthotropic, and Holzapfel forms of strain energy potential, toggle on Use temperature-dependent coefficients to define material parameters that depend on temperature.
A column labeled Temp appears in the data table.
If you are defining the hyperelastic behavior of a viscoelastic material, click the arrow to the right of the Moduli field to specify either Long-term or Instantaneous elastic response. See “Viscoelasticity” in “Anisotropic hyperelastic behavior,” Section 22.5.3 of the Abaqus Analysis User's Guide, for more information.
For the Holzapfel strain energy potential, click the arrows to the right of the Number of local directions field to increase or decrease the number of preferred local directions (or fiber directions) in the material. The default (and minimum) is 1. See “Creating an anisotropic hyperelastic material model” in “Defining elasticity,” Section 12.9.1 below and “Holzapfel-Gasser-Ogden form” in “Anisotropic hyperelastic behavior,” Section 22.5.3 of the Abaqus Analysis User's Guide, for more information.
For a user-defined strain energy potential, you must specify the following options:
Choose Strain or Invariant as the formulation defined by your user subroutine.
Choose Incompressible or Compressible as the type of material defined by your user subroutine. See “Compressibility” in “Anisotropic hyperelastic behavior,” Section 22.5.3 of the Abaqus Analysis User's Guide, for more information.
Specify the Number of property values needed as data in your user subroutine.
Enter the material parameters in the data table corresponding to the chosen strain energy potential.
Fung-Anisotropic
Holzapfel
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 create a hyperfoam material model to describe a cellular solid whose porosity permits very large volumetric changes. See “Hyperelastic behavior in elastomeric foams,” Section 22.5.2 of the Abaqus Analysis User's Guide, for more information on hyperfoam materials.
When you define a hyperfoam material, you have the option of either specifying material parameters directly or allowing Abaqus to calculate them from test data that you provide. For detailed instructions, see the following sections:
“Entering material parameters to define a hyperelastic foam material”
“Providing test data to define a hyperelastic foam material model”
You can provide the parameters of the hyperelastic foam strain energy potentials directly as functions of temperature.
To specify hyperelastic foam material parameters directly:
From the menu bar in the Edit Material dialog box, select MechanicalElasticityHyperfoam.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Click the arrows to the right of the Strain energy potential order field to increase or decrease the order of the strain energy potential, N.
To specify material parameters that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the Data table.
If you are defining the hyperfoam behavior of a viscoelastic material, click the arrow to the right of the Moduli time scale (for viscoelasticity) field to specify either long-term or instantaneous elastic response.
In the Data table, enter the material parameters: :
mui, alphai, and nui
Material parameters , , and 
.
Temp
Temperature.
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).
Abaqus can calculate material parameters from test data that you enter in the Test Data Editor.
To define a hyperelastic foam material by providing test data:
From the menu bar in the Edit Material dialog box, select MechanicalElasticityHyperfoam.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Toggle on Use test data (Suboptions must be specified).
Click the arrows to the right of the Strain energy potential order field to increase or decrease the order of the strain energy potential, N.
Indicate how you want to define Poisson effects:
Toggle on Use constant Poisson's ratio if you want to enter a Poisson's ratio that will remain constant throughout the calculations.
Toggle off Use constant Poisson's ratio if you want Poisson effects defined from volumentric test data and/or lateral strains in other test data.
If you are defining the hyperfoam behavior of a viscoelastic material, click the arrow to the right of the Moduli time scale (for viscoelasticity) field to specify either long-term or instantaneous elastic response.
Use the Test Data menu to specify the experimental data from which Abaqus can calculate material parameters. For detailed instructions, see the following sections:
“Specifying uniaxial test data for a hyperelastic foam material model”
“Specifying biaxial test data for a hyperelastic foam material model”
“Specifying simple shear test data for a hyperelastic foam material model”
“Specifying planar test data for a hyperelastic foam material model”
“Specifying volumetric test data for a hyperelastic foam material model”
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 Test Data Editor to specify uniaxial test data from which Abaqus can calibrate hyperelastic foam material coefficients. For more information, see “Hyperelastic behavior in elastomeric foams,” Section 22.5.2 of the Abaqus Analysis User's Guide.
To specify uniaxial test data:
Create a hyperelastic foam material model as described in “Providing test data to define a hyperelastic foam material model.”
From the Suboptions menu in the Edit Material dialog box, select Uniaxial Test Data.
A Test Data Editor appears.
In the Data table, enter the uniaxial test data:
Nominal Stress
Nominal stress, .
Nominal Strain
Nominal strain, .
Lateral Nominal Strain
Nominal lateral strain, . This parameter is unnecessary if you have already entered a constant Poisson's ratio in the Edit Material dialog box.
Click OK to return to the Edit Material dialog box.
Use the Test Data Editor to specify biaxial test data from which Abaqus can calibrate hyperfoam material coefficients. For more information, see “Hyperelastic behavior in elastomeric foams,” Section 22.5.2 of the Abaqus Analysis User's Guide.
To specify biaxial test data:
Create a hyperelastic foam material model as described in “Providing test data to define a hyperelastic foam material model.”
From the Suboptions menu in the Edit Material dialog box, select Biaxial Test Data.
A Test Data Editor appears.
In the Data table, enter the test data:
Nominal Stress
Nominal stress, 
.
Nominal Strain
Nominal strain, .
Lateral Nominal Strain
Nominal transverse strain, . This parameter is unnecessary if you have already entered a constant Poisson's ratio in the Edit Material dialog box.
Click OK to return to the Edit Material dialog box.
Use the Test Data Editor to specify simple shear test data from which Abaqus can calibrate hyperfoam material coefficients. For more information, see “Hyperelastic behavior in elastomeric foams,” Section 22.5.2 of the Abaqus Analysis User's Guide.
To specify simple shear test data:
Create a hyperelastic foam material model as described in “Providing test data to define a hyperelastic foam material model.”
From the Suboptions menu in the Edit Material dialog box, select Simple Shear Test Data.
A Test Data Editor appears.
In the Data table, enter the test data:
Nominal Stress
Nominal shear stress, .
Nominal Strain
Nominal shear strain, 
.
Nominal transverse stress
Nominal transverse stress, 
(normal to edge with shear stress). This stress value is optional, but strongly recommended. If given, a more accurate material response will be obtained.
Click OK to return to the Edit Material dialog box.
Use the Test Data Editor to specify planar test data from which Abaqus can calibrate hyperfoam material coefficients. Planar test data alone is inadequate; you must also include uniaxial and/or biaxial test data in the material definition. See the following sections for more information:
“Hyperelastic behavior in elastomeric foams,” Section 22.5.2 of the Abaqus Analysis User's Guide
“Specifying uniaxial test data for a hyperelastic foam material model”
“Specifying biaxial test data for a hyperelastic foam material model”
To specify planar test data:
Create a hyperelastic foam material model as described in “Providing test data to define a hyperelastic foam material model.”
From the Suboptions menu in the Edit Material dialog box, select Planar Test Data.
A Test Data Editor appears.
In the Data table, enter the test data:
Nominal Stress
Nominal stress, .
Nominal Strain
Nominal strain in the direction of loading, 
.
Nominal Lateral Strain
Nominal transverse strain, . This parameter is unnecessary if you have already entered a constant Poisson's ratio in the Edit Material dialog box.
Click OK to return to the Edit Material dialog box.
Use the Test Data Editor to specify volumetric test data from which Abaqus can calibrate hyperfoam material coefficients. For more information, see “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
To specify volumetric test data:
Create a hyperelastic foam material model as described in “Providing test data to define a hyperelastic foam material model.”
From the Test Data menu in the Edit Material dialog box, select Volumetric Test Data.
A Test Data Editor appears.
In the Data table, enter the test data:
Pressure
Pressure, p.
Volume Ratio
Volume ratio (current volume/original volume), J.
Click OK to return to the Edit Material dialog box.
You can create a material model to describe a low-density, highly compressible elastomeric foam with significant rate-sensitive behavior (such as polyurethane foam). Abaqus calculates material parameters from test data that you enter in the Test Data Editor. You must provide uniaxial test data for both tension and compression. Your test data must specify the uniaxial stress-strain curve for different strain-rate values.
See “Specifying low-density foam material properties,” for details about how to specify the material properties of a low-density foam.
Enter the properties in the Edit Material dialog box, as described below. See “Low-density foams,” Section 22.9.1 of the Abaqus Analysis User's Guide, for more information on low-density foam materials.
To specify low-density foam material properties:
From the menu bar in the Edit Material dialog box, select MechanicalElasticityLow Density Foam.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Select the Strain rate measure.
Choose Volumetric (default) to use the nominal volumetric strain rate that does not produce rate-sensitive behavior under volume-preserving deformation modes (e.g., simple shear).
Choose Principal to cause Abaqus to use the strain rate evaluated along each principal direction.
See “Strain rate” in “Low-density foams,” Section 22.9.1 of the Abaqus Analysis User's Guide, for more details.
Toggle on Extrapolate stress-strain curve beyond maximum strain rate to activate strain-rate extrapolation based on slope (with respect to the strain rate). See “Extrapolation of stress-strain curves” in “Low-density foams,” Section 22.9.1 of the Abaqus Analysis User's Guide, for more details.
Toggle on Maximum allowable principal tensile stress to enter a cutoff value that the foam material can sustain. The maximum principal tensile stresses computed by Abaqus will be forced to stay at or below this value. See “Tension cutoff and failure” in “Low-density foams,” Section 22.9.1 of the Abaqus Analysis User's Guide, for more details.
If you specified a value for the Maximum allowable principal tensile stress, toggle on Remove elements exceeding maximum to cause Abaqus to delete any elements in which the maximum principal tensile stress is reached. This is a simple method for modeling rupture.
You can accept the default values for Relaxation coefficients or enter new values for mu0, mu1, and alpha. See “Relaxation coefficients” in “Low-density foams,” Section 22.9.1 of the Abaqus Analysis User's Guide, for a detailed description of these material parameters.
To define the uniaxial test data for the material, click Uniaxial Test Data. For details, see the following sections:
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 Test Data Editor to specify uniaxial test data for tension.
To specify uniaxial tension test data:
Create a low-density foam material model as described in “Specifying low-density foam material properties.”
From the Uniaxial Test Data menu in the Edit Material dialog box, select Uniaxial Tension Test Data.
A Test Data Editor appears.
To specify test data that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the Data table.
To specify test 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.
Field variable columns appear in the Data table.
In the Data table, enter the test data:
Nominal Stress
Nominal stress, .
Nominal Strain
Nominal strain, .
Nominal Strain Rate
Nominal strain rate, 
. (Provide positive values to specify the loading response and negative values to specify unloading.)
Temp
Temperature, .
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
Use the Test Data Editor to specify uniaxial test data for compression.
To specify uniaxial compression test data:
Create a low-density foam material model as described in “Specifying low-density foam material properties.”
From the Uniaxial Test Data menu in the Edit Material dialog box, select Uniaxial Compression Test Data.
A Test Data Editor appears.
To specify test data that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the Data table.
To specify test 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.
Field variable columns appear in the Data table.
In the Data table, enter the test data:
Nominal Stress
Enter the absolute value of nominal stress, .
Nominal Strain
Enter the absolute value of nominal strain, .
Nominal Strain Rate
Nominal strain rate, . (Provide positive values to specify the loading response and negative values to specify unloading.)
Temp
Temperature, .
Field n
Predefined field variables.
Click OK to return to the Edit Material dialog box.
You can create a hypoelastic material definition to describe a nonlinear, small-strain elastic material. You have the option of either entering hypoelastic material parameters directly in the material editor or defining material parameters in user subroutine UHYPEL. User subroutine UHYPEL allows you to specify temperature-dependent data.
For more information, see the following sections:
“Hypoelastic behavior,” Section 22.4.1 of the Abaqus Analysis User's Guide
“UHYPEL,” Section 1.1.40 of the Abaqus User Subroutines Reference Guide
To create a hypoelastic material:
From the menu bar in the Edit Material dialog box, select MechanicalElasticityHypoelastic.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Select one of the following options for specifying material parameters:
Toggle on Use user subroutine UHYPEL.
Enter material parameters in the Data area:
Young's Modulus
Instantaneous Young's modulus, E.
Poisson's Ratio
Instantaneous Poisson's ratio, .
I1
First strain invariant, 
.
I2
Second strain invariant, 
.
I3
Third strain invariant, 
.
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).
A porous elastic material model defines the elastic parameters for a porous material. For more information, see “Elastic behavior of porous materials,” Section 22.3.1 of the Abaqus Analysis User's Guide.
To define a porous elastic material:
From the menu bar in the Edit Material dialog box, select MechanicalElasticityPorous Elastic.
(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 field and select an option for defining deviatoric elastic behavior in the porous material:
Select G to specify a constant shear modulus. In this case the shear behavior is unaffected by compaction of the material.
A Shear Modulus column appears in the Data table.
Select Poisson to allow Abaqus to calculate the instantaneous shear modulus from the bulk modulus and Poisson's ratio. In this case, the elastic shear stiffness increases as the material is compacted.
A Poisson's ratio column appear in the Data table.
To define behavior data that depend on temperature, toggle on Use temperature-dependent data.
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.
Field variable columns appear in the Data table.
In the Data table, enter the material parameters:
Log Bulk Modulus
Logarithmic bulk modulus, 
. (Dimensionless.)
G
Shear modulus, G. Enter this value if you selected G from the list of Shear options.
Poisson's ratio
Poisson's ratio, . Enter this value if you selected Poisson from the list of Shear options.
Tensile Limit
Elastic tensile limit, 
. (This value cannot be negative.)
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 define viscoelastic behavior in a material as a function of frequency (for steady-state, small-vibration analyses) or as a function of reduced time (for time-dependent analyses). For more information, see the following sections:
For detailed instructions on defining viscoelasticity in the Edit Material dialog box, see the following sections:
For more information on viscoelasticity, see “Time domain viscoelasticity,” Section 22.7.1 of the Abaqus Analysis User's Guide, and “Defining frequency domain viscoelasticity.This type of material model describes the isotropic rate-dependent behavior of materials for which the dissipative losses caused by internal damping effects must be modeled in the time domain.
Abaqus assumes that the time domain viscoelasticity is defined by a Prony series expansion. You can specify the Prony series parameters directly for each term in the Prony series. Alternatively, Abaqus can calculate the terms in the Prony series using time-dependent creep test data, time-dependent relaxation test data, or frequency-dependent cyclic test data that you provide.
For more information on time domain viscoelasticity, see “Time domain viscoelasticity,” Section 22.7.1 of the Abaqus Analysis User's Guide.
To define time domain viscoelasticity:
From the menu bar in the Edit Material dialog box, select MechanicalElasticityViscoelastic.
(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 Domain field, and select Time.
Click the arrow to the right of the Time field, and select the option of your choice for determining viscoelastic material parameters:
Select Prony if you want to enter the Prony series parameters for each term directly.
Select Creep test data if you want Abaqus to calculate the parameters in the Prony series from creep test data that you provide. If you select this option, you must enter shear test data and/or volumetric test data in the Test Data Editor.
Select Relaxation test data if you want Abaqus to calculate the Prony series parameters from relaxation test data. If you select this option, you must enter shear test data and/or volumetric test data in the Test Data Editor.
Select Frequency data if you want Abaqus to calculate the Prony series parameters from frequency-dependent cyclic test data.
If you selected any of the test data options from the Time option list, you can specify two additional parameters related to the calibration of Prony series parameters:
Click the arrows to the right of the Maximum number of terms in the Prony series field to specify the maximum number of terms (N) in the Prony series. Abaqus will perform the least-squares fit from 
to 
NMAX until convergence is achieved for the lowest N with respect to the error tolerance.
In the Allowable average root-mean-square error field, enter the error tolerance for the data points in the least-squares fit.
If you selected Prony from the list of Time options, enter the Prony parameters in the Data table.
g_i Prony
Shear relaxation or shear traction relaxation modulus ratio, 
.
k_i Prony
Bulk relaxation or normal traction relaxation modulus ratio, 
.
tau_i Prony
Relaxation time, 
.
If you selected Frequency data from the list of Time options, enter the frequency-dependent test data in the Data table.
Omega g* real
Real part of 
.
Omega g* imag
Imaginary part of .
Omega k* real
Real part of 
.
Omega k* imag
Imaginary part of .
Frequency
Frequency, f, in cycles per time.
If applicable, click Test Data to specify test data from which to define viscoelastic behavior. See the following sections for details:
To specify thermo-rheologically simple (TRS) temperature effects, use the Suboptions menu. For details, see “Specifying thermo-rheologically simple (TRS) temperature dependence for time domain viscoelasticity.”
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 shift function either by entering parameters for the Williams-Landel-Ferry approximation or by using user subroutine UTRS. For more information on temperature effects in time domain viscoelasticity, see “Time domain viscoelasticity,” Section 22.7.1 of the Abaqus Analysis User's Guide.
To define the shift function:
Create a time domain viscoelastic material as described in “Defining time domain viscoelasticity.”
From the Suboptions menu in the Edit Material dialog box, select Trs.
The Suboption Editor appears.
Click the arrow to the right of the Shift function field, and select the option of your choice.
Select WLF to define the shift function using the Williams-Landel-Ferry approximation.
Select User Subroutine UTRS to define the shift function using user subroutine UTRS.
If you selected WLF from the list of Shift function options, enter the required data in the Data table:
Theta 0
Reference temperature, 
.
C1
Calibration constant, 
.
C2
Calibration constant, 
.
Click OK to return to the Edit Material dialog box.
This type of material model describes frequency-dependent material behavior in small, steady-state harmonic oscillations. In these cases the dissipative losses caused by internal damping effects must be modeled in the frequency domain.
The dissipative part of the material behavior is defined by giving the real and imaginary parts of 
and 
(for compressible materials) as functions of frequency. The moduli can be defined as functions of the frequency in one of three ways: by a power law, by tabular input, or by a Prony series expression for the shear and bulk relaxation moduli.
For more information on frequency domain viscoelasticity, see “Frequency domain viscoelasticity,” Section 22.7.2 of the Abaqus Analysis User's Guide.
To define frequency domain viscoelasticity:
From the menu bar in the Edit Material dialog box, select MechanicalElasticityViscoelastic.
(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 Domain field, and select Frequency.
Click the arrow to the right of the Frequency field, and select the option of your choice for determining viscoelastic material parameters:
Select Formula to define the frequency dependence by the power law formulae.
Select Tabular to define the frequency response in tabular form. You must provide the real and imaginary parts of and —where 
is the circular frequency—as functions of frequency in cycles per time.
Select Prony if you want Abaqus to calculate the frequency dependence from a time domain Prony series description of the dimensionless shear and bulk relaxation moduli.
Select Creep test data if you want Abaqus to calculate the parameters in the Prony series from creep test data that you provide. If you select this option, you must enter shear test data and/or volumetric test data in the Test Data Editor.
Select Relaxation test data if you want Abaqus to calculate the Prony series parameters from relaxation test data. If you select this option, you must enter shear test data and/or volumetric test data in the Test Data Editor.
If you selected Creep test data or Relaxation test data from the Frequency option list, you can specify two additional parameters related to the calibration of Prony series parameters:
Click the arrows to the right of the Maximum number of terms in the Prony series field to specify the maximum number of terms (N) in the Prony series. Abaqus will perform the least-squares fit from to NMAX until convergence is achieved for the lowest N with respect to the error tolerance.
In the Allowable average root-mean-square error field, enter the error tolerance of the data points in the least-squares fit.
If you selected Tabular from the Frequency option list, you can specify two additional options:
Type
This parameter specifies whether you are defining continuum material properties or effective thickness-direction gasket properties.
Select Isotropic if you are defining continuum material properties. This choice is appropriate when the viscoelasic material model is used for any continuum, structural, or special-purpose elements whose material response is modeled using continuum material properties.
Select Traction if you are defining effective thickness-direction gasket properties. This option is supported only for gasket elements whose behavior is modeled directly using a gasket behavior model.
Preload
This parameter specifies the nature of preload used for defining frequency domain viscoelastic material properties or effective thickness-direction gasket properties.
Select Uniaxial to specify that the material properties correspond to a uniaxial test.
Select Volumetric to specify that the material properties correspond to a volumetric test. This setting cannot be used to define effective thickness-direction gasket properties.
Select Uniaxial and Volumetric to specify that the material properties correspond to both types of tests. This setting cannot be used to define effective thickness-direction gasket properties.
Select None if you choose not to specify a preload parameter.
If you selected Formula from the list of Frequency options, enter the following data in the Data table:
g1*real
Real part of 
.
g1*imag
Imaginary part of .
a
Value of a.
k1*real
Real part of 
.
k1*imag
Imaginary part of . If the material is incompressible, this value is ignored.
b
Value of b. If the material is incompressible, this value is ignored.
If you selected Tabular from the list of Frequency options, enter the data relevant to your Type and Preload selections (not all of the following parameters will apply):
Omega g* real
Real part of . 
Omega g* imag
Imaginary part of . 
Omega k* real
Real part of . 
If the material is incompressible, this value is ignored.
Omega k* imag
Imaginary part of . 
If the material is incompressible, this value is ignored.
Frequency
Frequency, f, in cycles per time.
Loss Modulus
Uniaxial or bulk loss modulus.
Storage Modulus
Uniaxial or bulk storage modulus.
Uniaxial Strain
Uniaxial nominal strain (defines the level of uniaxial preload).
Volume Ratio
Volume ratio, J (current volume/original volume; defines the level of volumetric preload).
Normalized Loss Modulus
Real part of . for thickness-direction gasket behavior with no preload.
Normalized Shear Modulus
Imaginary part of . for thickness-direction gasket behavior with no preload.
If you selected Prony from the list of Frequency options, enter the following data in the Data table:
g_i Prony
, the modulus ratio in the first term in the Prony series expansion of the shear relaxation modulus.
k_i Prony
, the modulus ratio in the first term in the Prony series expansion of the bulk relaxation modulus.
tau_i Prony
, the relaxation time for the first term in the Prony series expansion.
If applicable, use the Test Data menu to specify test data from which to define viscoelastic behavior. 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).
You can use the Test Data Editor to specify the normalized shear creep compliance or relaxation modulus as a function of time. For information on using shear test data to define viscoelastic material behavior, see “Time domain viscoelasticity,” Section 22.7.1 of the Abaqus Analysis User's Guide, or “Frequency domain viscoelasticity,” Section 22.7.2 of the Abaqus Analysis User's Guide.
To specify shear test data:
Create a viscoelastic material model as described in “Defining time domain viscoelasticity” or “Defining frequency domain viscoelasticity.”
From the Test Data menu in the Edit Material dialog box, select Shear Test Data.
A Test Data Editor appears.
In the Long-term normalized shear compliance or modulus field, enter either the long-term, normalized shear compliance, 
, for creep test data or the long-term, normalized shear modulus, 
, for relaxation test data.
In the Data table, enter the following data:
js or gR
The normalized shear compliance, 
, ( 
) for creep test data or the normalized shear relaxation modulus, 
, ( 
) for relaxation test data.
Time
Time, t. 
Click OK to return to the Edit Material dialog box.
You can use the Test Data Editor to specify the normalized bulk creep compliance or relaxation modulus as a function of time. For information on using volumetric test data to define viscoelastic material behavior, see “Time domain viscoelasticity,” Section 22.7.1 of the Abaqus Analysis User's Guide, or “Frequency domain viscoelasticity,” Section 22.7.2 of the Abaqus Analysis User's Guide.
To specify volumetric test data:
Create a viscoelastic material model as described in “Defining time domain viscoelasticity” or “Defining frequency domain viscoelasticity.”
From the Test Data menu in the Edit Material dialog box, select Volumetric Test Data.
A Test Data Editor appears.
In the Long-term normalized volumetric compliance or modulus field, enter either the long-term, normalized volumetric compliance, 
, for creep test data or the long-term, normalized volumetric modulus, 
, for relaxation test data.
In the Data table, enter the following data:
jK or kR
The normalized volumetric compliance, 
, for creep test data or the normalized volumetric modulus, 
, for relaxation test data.
Time
Time, t.
Click OK to return to the Edit Material dialog box.
You can use the Test Data Editor to specify simultaneously the normalized shear and bulk creep compliances or relaxation moduli as a function of time. For information on using combined test data to define viscoelastic material behavior, see “Time domain viscoelasticity,” Section 22.7.1 of the Abaqus Analysis User's Guide, or “Frequency domain viscoelasticity,” Section 22.7.2 of the Abaqus Analysis User's Guide.
To specify combined test data:
Create a viscoelastic material model as described in “Defining time domain viscoelasticity” or “Defining frequency domain viscoelasticity.”
From the Test Data menu in the Edit Material dialog box, select Combined Test Data.
A Test Data Editor appears.
In the Long-term normalized shear compliance or modulus field, enter either the long-term, normalized shear compliance, , for creep test data or the long-term, normalized shear modulus, , for relaxation test data.
In the Long-term normalized volumetric compliance or modulus field, enter either the long-term, normalized volumetric compliance, , for creep test data or the long-term, normalized volumetric modulus, , for relaxation test data.
In the Data table, enter the following data:
js or gR
The normalized shear compliance, , ( ) for creep test data or the normalized shear relaxation modulus, , ( ) for relaxation test data.
jK or kR
The normalized volumetric compliance, , for creep test data or the normalized volumetric modulus, , for relaxation test data.
Time
Time, t.
Click OK to return to the Edit Material dialog box.
, 
, 
, 
, 
, 
, 
, 
, 
, 
, 
, 
, 
, 
, 
, 
, 
, 
, 
, 
, 
, 
(units of 
(units of 
(units of 
, and the fiber dispersion parameter 
).