Specify linear elasticity by entering a Young's modulus and Poisson's ratio. Linear elasticity is intended for use with small elastic strains (normally less than 5%).

Specify plasticity by entering corresponding stress and strain values. You can choose isotropic, kinematic, or Johnson-Cook hardening. You must provide tabular data of stresses, strains, and temperatures to define isotropic or kinematic hardening.

Johnson-Cook hardening is a particular form of isotropic hardening that can be used only in an Abaqus Explicit Dynamics case. For Johnson-Cook hardening you must provide the melting and transition temperatures of the material and several material parameters.

For more information on plasticity, see Metal plasticity in the Abaqus Materials Guide.

You can define hyperelasticity for isotropic, nonlinear materials that exhibit an instantaneous elastic response to large strains. To use hyperelastic materials in an analysis, you must include geometric nonlinearity in the analysis steps. Analysis steps automatically include geometric nonlinearity when the model uses hyperelastic materials.

Hyperelasticity is defined by selecting one of the following strain energy potentials:

• Arruda-Boyce

• Mooney-Rivlin

• Neo Hooke

• Ogden

• Polynomial

• Reduced Polynomial

• Van der Waals

• Yeoh

After selecting a strain energy potential, you enter the coefficient data that Abaqus uses to calculate the material response. For more information on hyperelasticity and the formulas and coefficients associated with each strain energy potential, see Hyperelastic behavior of rubberlike materials in the Abaqus Materials Guide.

Specify the density for use with gravity loads or when conducting a heat transfer analysis.

Specify the thermal conductivity for use in a heat transfer analysis.

Specify the specific heat for use in a heat transfer analysis.

Specify the coefficient of thermal expansion if you intend to run a thermal analysis and use the results as the basis for a subsequent structural analysis.

A user-defined material allows you to supply constants for use in defining your own general material model. The constants are used by Abaqus for CATIA V5 in an Abaqus user subroutine to define the mechanical or thermal constitutive behavior of the material under the current analysis conditions. In addition to supplying the required constants, you must also program a user subroutine to use them and provide the path to the subroutine file when you create the job (see Using User Subroutines). For more information on user-defined materials, see User materials in the Abaqus Materials Guide. If you select User-defined Material, the material definition that you create overrides all other Abaqus material properties.

Specify a volumetric heat generation within a material for use in a heat transfer analysis. You define the heat generation in user subroutine HETVAL and provide the path to the subroutine file when you create the job (see Using User Subroutines). There are no additional data required for this property. For more information, see Internal heat generation in Uncoupled heat transfer analysis in the Abaqus Analysis Guide.

Specify the gasket material properties. You must define the thickness loading behavior in terms of pressure and closure data, where the closure between the top and bottom faces of a gasket element is the thickness-direction deformation. You can also choose between elastic-plastic and damage elasticity loading models. Both models allow you to select a tensile stiffness factor and include temperature-dependent data and field variables. The elastic-plastic model also allows you to define the onset of yield using a percentage drop in the slope of the loading curve from its maximum value—the default drop is 0.1 or 10%—or a closure value.

You can also add thickness unloading, transverse shear, and membrane behavior to the gasket material definition. If you define an unloading curve, it uses the same model (elastic-plastic or damage) as the loading curve and is used in addition to the default unloading curve—the scaled portion of the loading curve before the point of yield onset. For more information, see Defining the gasket behavior directly using a gasket behavior model in the Abaqus Elements Guide.