Defining the gasket behavior using a material model

The gasket behavior defined by a material model:

  • can be specified in terms of a built-in material model or a user-defined small-strain material model;

  • considers only the thickness behavior and assumes a uniaxial stress state for gasket elements that model thickness-direction behavior only;

  • admits both compressive and tensile stresses in the thickness direction;

  • is defined in terms of small-strain measures and, hence, finite-strain material models such as hyperelastic and hyperfoam cannot be used;

  • is restricted to small-strain elasticity models for line gasket elements that use the built-in material models;

  • causes Abaqus/Standard to use the reference thickness to convert the relative displacements at the top and bottom surfaces of the gasket to strains and uses these strains in conjunction with the constitutive law to obtain the stresses; and

  • makes the notions of “initial gap” and “initial void” in the thickness direction irrelevant (consequently, Abaqus/Standard ignores such data specified as part of the gasket section property definition).

The following topics are discussed:

Related Topics
About gasket elements
In Other Guides
UMAT
Creating and editing materials

ProductsAbaqus/StandardAbaqus/CAE

Assigning a gasket behavior to a gasket element

To define the gasket behavior by a material model, you must assign a gasket section definition to a region of your model and assign the name of a material definition to the gasket section definition. The gasket behavior for this region is defined entirely by the gasket thickness and the material properties specified by the material definition referring to the same name.

The gasket behavior can be defined in terms of a built-in or a user-defined material model. In the latter case the actual material model is defined in user subroutine UMAT.

Input File Usage

Use the following options to define the gasket behavior in terms of a built-in material model:

GASKET SECTION, ELSET=name, MATERIAL=name
MATERIAL, NAME=name

Use the following options to define the gasket behavior in terms of a user-defined material model:

GASKET SECTION, ELSET=name, MATERIAL=name
MATERIAL, NAME=name
USER MATERIAL, CONSTANTS=n

Abaqus/CAE Usage

Property module: 
Create Material: Name: name, enter data for any materials that are valid for 
gasket sections except those found under OtherGasket
Create Section: select Other as the section Category and Gasket as the section Type: Material: name

Tensile behavior modeling

Tensile behavior modeling can be desirable when gaskets carry (limited) tensile stresses, such as occurs when adhesives are present. Undesired tensile behavior can be avoided by using appropriate contact pairs and/or implementing a user-defined no-tension material model in user subroutine UMAT.

Specific output for material definition of gasket behavior

The output variables for stresses and strains are the same as those used for solid elements: tensile and compressive stresses/strains are indicated as positive and negative quantities, respectively. However, for all stress/strain output variables the 11-component refers to the through-thickness direction; the 22-, 33-, and 23-components refer to two direct and one shear membrane component, respectively; the remaining 12- and 13-components refer to the transverse shear components. For details about these definitions, see About gasket elements. The output variable NE is available to output nominal (effective) strains for gasket elements defined using a material model; however, NE is identical to E in this case.