Hypoelastic Behavior

The hypoelastic model in Abaqus/Standard 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.

The hypoelastic material model:

  • is valid for small elastic strains—the stresses should not be large compared to the elastic modulus of the material;

  • is used when the load path is monotonic; and

  • must be defined by user subroutine UHYPEL if temperature dependence is to be included.

This page discusses:

See Also
About the Material Library
Elastic Behavior
In Other Guides
*HYPOELASTIC

Products Abaqus/Standard

Defining Hypoelastic Material Behavior

In a hypoelastic material the rate of change of stress is defined as a tangent modulus matrix multiplying the rate of change of the elastic strain:

d ⁢ σ = D e ⁢ l : d ⁢ ε e ⁢ l ,

where d⁢σ is the rate of change of the stress (the “true,” Cauchy, stress in finite-strain problems), De⁢l is the tangent elasticity matrix, and d⁢εe⁢l is the rate of change of the elastic strain (the log strain in finite-strain problems).

Determining the Hypoelastic Material Parameters

The entries in De⁢l are provided by giving Young's modulus, E, and Poisson's ratio, ν, as functions of strain invariants. The strain invariants are defined for this purpose as

I 1 = ​ trace ⁢ ε e ⁢ l , I 2 = ​ 1 2 ( ε e ⁢ l : ε e ⁢ l - I 1 2 ) , I 3 = ​ det ⁢ ( ε e ⁢ l ) .

You can define the material parameters directly or by using a user subroutine.

Direct Specification

You can define the variation of Young's modulus and Poisson's ratio directly by specifying E, ν, I1, I2, and I3.

Input File Usage

HYPOELASTIC

User Subroutine

If specifying E and ν as functions of the strain invariants directly does not allow sufficient flexibility, you can define the hypoelastic material by user subroutine UHYPEL.

Input File Usage

HYPOELASTIC, USER

Plane or Uniaxial Stress

For plane stress and uniaxial stress states Abaqus/Standard does not compute the out-of-plane strain components. For the purpose of defining the above invariants, it is assumed that I1= 0; that is, the material is assumed to be incompressible. For example, in a uniaxial stress case (such as a truss element) this assumption implies that

I 1 = ​ 0 , I 2 = ​ 3 4 ⁢ ( ε 11 e ⁢ l ) 2 , I 3 = ​ 1 4 ⁢ ( ε 11 e ⁢ l ) 3 .

Large-Displacement Analysis

For large-displacement analysis the strain measure in Abaqus is the integration of the rate of deformation. This strain measure corresponds to log strain if the principal directions do not rotate relative to the material. The strain invariant definitions should be interpreted in this way.

Material Options

The hypoelastic material model can be used only by itself in the material definition. It cannot be combined with viscoelasticity or with any inelastic response model. See Combining Material Behaviors for more details.

Elements

The hypoelastic material model can be used with any of the stress/displacement elements in Abaqus/Standard.