You use the Material Editor 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”
Hyperelastic; see “Creating a hyperelastic 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. “Specifying elastic material properties” discusses 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 10.2.1 of the ABAQUS Analysis User's Manual.
To specify elastic material properties:
From the main menu bar, select Material
Create.
In the Material Editor that appears, enter a name for the material.
From the menu bar in the Material Editor, select MechanicalElasticityElastic.
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 10.2.1 of the ABAQUS Analysis User's Manual.
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 10.2.1 of the ABAQUS Analysis User's Manual.
Choose Lamina to specify orthotropic elastic properties in plane stress, as described in “Defining orthotropic elasticity in plane stress” in “Linear elastic behavior,” Section 10.2.1 of the ABAQUS Analysis User's Manual.
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 10.2.1 of the ABAQUS Analysis User's Manual.
Choose Anisotropic to specify anisotropic elastic properties, as described in “Defining fully anisotropic elasticity” in “Linear elastic behavior,” Section 10.2.1 of the ABAQUS Analysis User's Manual.
Select the Moduli time scale that will be used if the linear elastic material model is used to specify the elastic response of a viscoelastic material model:
Select Instantaneous to indicate that the elastic material constants define the instantaneous behavior of the viscoelastic material. This choice is not valid for frequency domain viscoelasticity in an ABAQUS/Standard analysis.
Select Long-term to indicate that the elastic material constants define the long-term behavior of the viscoelastic material.
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.
Enter the material properties in the Data table.
For Isotropic data, enter the Young's modulus, 
, 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 nine elastic stiffness parameters: 
, 
, etc. (units of FL–2).
For Anisotropic data, enter the twenty-one elastic stiffness parameters: , , etc. (units of FL–2).
To define the plane stress orthotropic failure measures for the material, if desired, click Suboptions. For details, see:
Click OK to create the material and to exit the editor.
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 10.2.3 of the ABAQUS Analysis User's Manual.
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 Material Editor, select Fail Stress.
To define behavior data that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the tabular data area.
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 tabular data area.
In the Data table of the Suboption Editor that appears, enter the stress limits (you may need to expand the dialog box to see all the columns):
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 
–
plane, 
.
Cross-prod Term Coeff
Cross-product term coefficient, 
(
). This value is used only for the Tsai-Wu theory and is ignored if 
is given. 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 material editor.
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 10.2.3 of the ABAQUS Analysis User's Manual.
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 Material Editor, select Fail Strain.
To define behavior data that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the tabular data area.
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 tabular data area.
In the Data table of the Suboption Editor that appears, enter the strain limits (you may need to expand the dialog box to see all the columns):
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 – plane, 
.
Click OK to create the material to return to the material editor.
For rubberlike material at finite strain the hyperelastic model describes the material behavior for nearly incompressible elastomers. This nonlinear elasticity model is valid for large elastic strains. “Specifying hyperelastic material properties” discusses how to define a hyperelastic material model.
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:
Arruda-Boyce: The Arruda-Boyce model is also known as the eight-chain model. For more information, see “Arruda-Boyce form” in “Hyperelastic behavior,” Section 10.5.1 of the ABAQUS Analysis User's Manual.
Marlow: For more information, see “Marlow form” in “Hyperelastic behavior,” Section 10.5.1 of the ABAQUS Analysis User's Manual.
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,” Section 10.5.1 of the ABAQUS Analysis User's Manual.
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,” Section 10.5.1 of the ABAQUS Analysis User's Manual.
Ogden: For more information, see “Ogden form” in “Hyperelastic behavior,” Section 10.5.1 of the ABAQUS Analysis User's Manual.
Polynomial: For more information, see “Polynomial form” in “Hyperelastic behavior,” Section 10.5.1 of the ABAQUS Analysis User's Manual.
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,” Section 10.5.1 of the ABAQUS Analysis User's Manual.
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,” Section 10.5.1 of the ABAQUS Analysis User's Manual.
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,” Section 10.5.1 of the ABAQUS Analysis User's Manual.
Yeoh: The Yeoh model is equivalent to using the reduced polynomial model with N=3. For more information, see “Yeoh form” in “Hyperelastic behavior,” Section 10.5.1 of the ABAQUS Analysis User's Manual.
In addition, when you define a hyperelastic material using experimental data, you have the option of selecting Unknown as the Strain energy potential. This option allows you to define the material temporarily without specifying a particular strain energy potential. 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 12.4.6, for more information.The parameters of the hyperelastic strain energy potentials can be given directly as functions of temperature. Alternatively, the material coefficients of the hyperelastic models can be calibrated by ABAQUS from experimental stress-strain data. For more information, see “Hyperelastic behavior,” Section 10.5.1 of the ABAQUS Analysis User's Manual.
To specify a hyperelastic material model by specifying the material constants directly:
From the main menu bar, select MaterialCreate.
In the Material Editor that appears, enter a name for the material.
From the menu bar in the Material Editor, select MechanicalElasticityHyperelastic.
Select Coefficients as the Input source. This choice is not valid for the Marlow model or for an unknown strain energy potential; in these cases the test data must be specified.
From the Strain energy potential field, choose the strain energy potential.
Select the Moduli time scale that will be used if the hyperelastic material model is used to specify the elastic response of a viscoelastic or hysteretic material model:
Select Instantaneous to indicate that the hyperelastic material constants define the instantaneous behavior of the viscoelastic or hysteretic material. This choice is not valid for frequency domain viscoelasticity in an ABAQUS/Standard analysis. This is the only valid choice if the hyperelastic material is defined in user subroutine UHYPER.
Select Long-term to indicate that the hyperelastic material constants define the long-term behavior of the viscoelastic or hysteretic material. This choice is not valid if the hyperelastic material is defined in user subroutine UHYPER.
If you selected User-defined as the strain energy potential:
Toggle on Include compressibility to indicate that the material defined by user subroutine UHYPER is compressible. Otherwise, the material is assumed to be incompressible.
Specify the Number of property values needed as data in user subroutine UHYPER.
If you selected Ogden, Polynomial, or Reduced Polynomial as the strain energy potential, click the arrow next to the Strain energy potential order field and 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 
.
Mooney-Rivlin
Enter 
, 
, and 
.
Neo Hooke
Enter and .
Ogden
Enter 
, 
, and 
, where 
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 goes from 1 to N, and N is the value specified for the Strain energy potential order.
Reduced Polynomial
Enter 
and , where goes from 1 to N and N is the value specified for the Strain energy potential order.
Van der Waals
Enter , , 
, 
, and .
Yeoh
Enter , 
, 
, , 
, and 
.
Click OK to create the material and to exit the editor.
To specify a hyperelastic material model by providing test data:
From the main menu bar, select MaterialCreate.
In the Material Editor that appears, enter a name for the material.
From the menu bar in the Material Editor, select MechanicalElasticityHyperelastic.
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.
From the Strain energy potential field, choose the strain energy potential.
Select the Moduli time scale that will be used if the hyperelastic material model is used to specify the elastic response of a viscoelastic or hysteretic material model:
Select Instantaneous to indicate that the hyperelastic material constants define the instantaneous behavior of the viscoelastic or hysteretic material. This choice is not valid for frequency domain viscoelasticity in an ABAQUS/Standard analysis. This is the only valid choice if the hyperelastic material is defined in user subroutine UHYPER.
Select Long-term to indicate that the hyperelastic material constants define the long-term behavior of the viscoelastic or hysteretic material. This choice is not valid if the hyperelastic material is defined in user subroutine UHYPER.
If you selected Marlow as the strain energy potential, select the Data to define deviatoric response and the Data to define volumetric response.
The deviatoric response is defined by the Uniaxial, Biaxial, or Planar test data specified as described in Step 10.
The volumetric response is defined by one of the following methods:
Default: 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 10.
Poisson's ratio: Specify a value for the Poisson's ratio of the hyperelastic material.
Lateral nominal strain: Lateral nominal strains are specified as part of the uniaxial, biaxial, or planar test data, as described in Step 10.
If you selected Ogden, Polynomial, or Reduced Polynomial as the strain energy potential, click the arrow next to the Strain energy potential order field and 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.
The experimental stress-strain data can be specified for up to four simple tests: uniaxial, equibiaxial, planar, and, if the material is compressible, a volumetric compression test. Click Test Data to specify the experimental data.
Click OK to create the material and to exit the editor.