# Elastic behavior

 The material library in Abaqus includes several models of elastic behavior. The following topics are discussed:
Linear elasticity

Linear elasticity (Linear elastic behavior) 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.

Plane stress orthotropic failure

Failure theories are provided (Plane stress orthotropic failure measures) for use with linear elasticity. They can be used to obtain postprocessed output requests.

Porous elasticity

The porous elastic model in Abaqus/Standard (Elastic behavior of porous materials) is used for porous materials in which the volumetric part of the elastic strain varies with the logarithm of the equivalent pressure stress. This form of nonlinear elasticity is valid for small elastic strains.

Hypoelasticity

The hypoelastic model in Abaqus/Standard (Hypoelastic behavior) is used for materials in which the rate of change of stress is defined by an elasticity matrix multiplying the rate of change of elastic strain, where the elasticity matrix is a function of the total elastic strain. This general, nonlinear elasticity is valid for small elastic strains.

Rubberlike hyperelasticity

For rubberlike material at finite strain the hyperelastic model (Hyperelastic behavior of rubberlike materials) provides a general strain energy potential to describe the material behavior for nearly incompressible elastomers. This nonlinear elasticity model is valid for large elastic strains.

Foam hyperelasticity

The hyperfoam model (Hyperelastic behavior in elastomeric foams) provides a general capability for elastomeric compressible foams at finite strains. This nonlinear elasticity model is valid for large strains (especially large volumetric changes). The low-density foam model in Abaqus/Explicit (Low-density foams) is a nonlinear viscoelastic model suitable for specifying strain-rate sensitive behavior of low-density elastomeric foams such as used in crash and impact applications. The foam plasticity model (Crushable foam plasticity models) should be used for foam materials that undergo permanent deformation.

Anisotropic hyperelasticity

The anisotropic hyperelastic model (Anisotropic hyperelastic behavior) provides a general capability for modeling materials that exhibit highly anisotropic and nonlinear elastic behavior (such as biomedical soft tissues, fiber-reinforced elastomers, etc.). The model is valid for large elastic strains and captures the changes in the preferred material directions (or fiber directions) with deformation.

Fabric materials

The fabric model in Abaqus/Explicit (Fabric material behavior) for woven fabrics captures the directional nature of the stiffness along the fill and the warp yarn directions. It also captures the shear response as the yarn directions rotate relative to each other. The model takes into account finite strains including large shear rotations. It captures the highly nonlinear elastic response of fabrics through the use of test data or a user subroutine, VFABRIC (see VFABRIC) for the material characterization. The test data based fabric behavior can include nonlinear elasticity, permanent deformation, rate-dependent response, and damage accumulation.

Viscoelasticity

The viscoelastic model is used to specify time-dependent material behavior (Time domain viscoelasticity). In Abaqus/Standard it is also used to specify frequency-dependent material behavior (Frequency domain viscoelasticity). It must be combined with linear elasticity, rubberlike hyperelasticity, or foam hyperelasticity.

Parallel rheological framework

The parallel rheological framework (Parallel rheological framework) is intended for modeling nonlinear behavior for materials subjected to large strains, such as elastomers and polymers. The models defined within this framework consist of multiple parallel viscoelastic networks and, optionally, an elastoplastic network to allow modeling permanent set and material softening using the Mullins effect. The elastic response is defined using the hyperelastic material model; the plastic response is based on the theory of incompressible isotropic hardening plasticity; and the viscous response is specified using the flow rule derived from a creep potential.

Hysteresis

The hysteresis model in Abaqus/Standard (Hysteresis in elastomers) is used to specify rate-dependent behavior of elastomers. It is used in conjunction with hyperelasticity.

Mullins effect

The Mullins effect model (Mullins effect) is used to specify stress softening of filled rubber elastomers due to damage, a phenomenon referred to as Mullins effect. The model can also be used to include permanent energy dissipation and stress softening effects in elastomeric foams (Energy dissipation in elastomeric foams). It is used in conjunction with rubberlike hyperelasticity or foam hyperelasticity.

No compression or no tension elasticity

The no compression or no tension models in Abaqus/Standard (No compression or no tension) can be used when compressive or tensile principal stresses should not be generated. These options can be used only with linear elasticity.

## Thermal strain

Thermal expansion can be introduced for any of the elasticity or fabric models (Thermal expansion). ## Elastic strain magnitude

Except in the hyperelasticity and fabric material models, the stresses are always assumed to be small compared to the tangent modulus of the elasticity relationship; that is, the elastic strain must be small (less than 5%). The total strain can be arbitrarily large if inelastic response such as metal plasticity is included in the material definition.

For finite-strain calculations where the large strains are purely elastic, the fabric model (for woven fabrics), the hyperelastic model (for rubberlike behavior), or the foam hyperelasticity model (for elastomeric foams) should be used. The hyperelasticity and fabric models are the only models that give realistic predictions of actual material behavior at large elastic strains. The linear or, in Abaqus/Standard, porous elasticity models are appropriate in other cases where the large strains are inelastic.

In Abaqus/Standard the linear elastic, porous elastic, and hypoelastic models will exhibit poor convergence characteristics if the stresses reach levels of 50% or more of the elastic moduli; this limitation is not serious in practical cases because these material models are not valid for the resulting large strains.