<!-- source-page: 941 -->

![](images/page-941_adcfc1388761dbf75f4d7ea6d87a38dfb690c53c1dcfc3d67ac7a78b1c8a0620.jpg)

<details>
<summary>text_image</summary>

initial gap
metallic plate
metallic frame
initial void
spacers
</details>

Figure 32.6.4–6 Schematic representation of an initial gap and an initial void in a typical gasket.

# Stability of unsupported gasket elements

Gasket elements that extend outside neighboring components (unsupported gasket elements) can be troublesome and should be avoided. If a gasket element is completely or partially unsupported, incorrect areas can result in an incorrect stiffness, and numerical singularity problems can occur in the equation solver. Minor extensions (caused by numerical roundoff in mesh generation) will not usually cause a problem because Abaqus/Standard automatically extends the master surfaces a small amount beyond the edge of the model. Numerical problems can occur in the direction tangential to the gasket (if general gasket elements are used and no membrane stiffness is specified) as well as in the direction normal to the gasket. The numerical singularity problems normal to the gasket can be treated by stabilizing the elements with a small artificial stiffness. By default, Abaqus/Standard automatically applies a small stabilization stiffness (on the order of $1 0 ^ { - 9 }$ times the initial compressive stiffness in the thickness direction) to all types of gasket elements except the link elements. For persistent numerical singularity problems in unsupported gasket elements the following treatment methods can be considered. First, make sure that an adequate membrane elasticity is specified. Second, specify a higher value for the artificial stiffness for the gasket section. If problems still persist, consider trimming, “skinning,” and using MPCs (see “General multi-point constraints,” Section 35.2.2).

Input File Usage: Use the following option to change the artificial stiffness for a gasket section: \*GASKET SECTION, STABILIZATION STIFFNESS=stiffness\_value

Abaqus/CAE Usage: Use the following option to change the artificial stiffness for a gasket section: Property module: Create Section: select Other as the section Category and Gasket as the section Type: Stabilization stiffness: Specify: stiffness\_value

<!-- source-page: 942 -->

<!-- source-page: 943 -->

# 32.6.5 DEFINING THE GASKET BEHAVIOR USING A MATERIAL MODEL

Products: Abaqus/Standard Abaqus/CAE

# References

• “Gasket elements: overview,” Section 32.6.1   
• “UMAT,” Section 1.1.44 of the Abaqus User Subroutines Reference Guide   
• “Creating and editing materials,” Section 12.7 of the Abaqus/CAE User’s Guide, in the HTML version of this guide

# Overview

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).

# 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

<!-- source-page: 944 -->

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

```txt
*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 Other→Gasket

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 “Gasket elements: overview,” Section 32.6.1. 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.

<!-- source-page: 945 -->

# 32.6.6 DEFINING THE GASKET BEHAVIOR DIRECTLY USING A GASKET BEHAVIOR MODEL

Products: Abaqus/Standard Abaqus/CAE

# References

• “Gasket elements: overview,” Section 32.6.1   
• “Defining the gasket element’s initial geometry,” Section 32.6.4   
• “Defining gasket behavior,” Section 12.12.4 of the Abaqus/CAE User’s Guide, in the HTML version of this guide

# Overview

The gasket behavior defined by a gasket behavior model:

• can be specified in terms of uncoupled thickness direction, membrane, and transverse shear behavior only;   
• can be nonlinear elastic with damage or nonlinear elastic-plastic in the thickness direction;   
• can consider creep effects in the thickness direction when rate-independent elastic-plastic modeling is used;   
• can consider the dynamic stiffness and damping characteristics in the thickness direction when elastic-damage modeling is used;   
• will be linear elastic in the membrane and transverse shear directions; and   
• can consider thermal effects in the thickness and membrane directions.

# Assigning a gasket behavior to a gasket element

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

Input File Usage:

Use both of the following options to define the gasket behavior in terms of a gasket behavior model:

\*GASKET SECTION, ELSET=name, BEHAVIOR=name

\*GASKET BEHAVIOR, NAME=name

Abaqus/CAE Usage:

Property module:

Material editor: Name: name, enter data for any materials found under

Other→Gasket

Create Section: select Other as the section Category and Gasket

as the section Type: Material: name

<!-- source-page: 946 -->

# Specifying a gasket behavior

The thickness-direction, transverse shear, and membrane behaviors are defined to be uncoupled. Each behavior is specified independently.

You must specify the thickness-direction behavior. You can specify multiple thickness-direction behaviors to define the loading and unloading characteristics. You can obtain an average contact pressure output when the thickness-direction behavior is defined as force or force per unit length versus closure.

The transverse shear and membrane behaviors are optional for gasket elements that have all displacement degrees of freedom active at their nodes. You can define one or both of these behaviors.

When thermal and rate-dependent effects are important, you can define thermal expansion and creep behavior for gaskets; user subroutines UEXPAN and CREEP can be used to define these behaviors.

You cannot specify density for gasket elements since they have no mass matrix.

Input File Usage: Use the first two options and any of the following options to specify a gasket behavior:

\*GASKET BEHAVIOR, NAME=name   
\*GASKET THICKNESS BEHAVIOR   
\*GASKET ELASTICITY   
\*GASKET CONTACT AREA   
\*EXPANSION   
\*CREEP   
\*DEPVAR   
\*USER OUTPUT VARIABLES

The \*GASKET THICKNESS BEHAVIOR option can be repeated to define the loading and unloading characteristics of the thickness-direction behavior. The \*GASKET ELASTICITY option can be repeated to define both transverse shear and membrane behaviors. The other options cannot be repeated within a single behavior definition. The order in which these options are specified has no importance, but they must appear immediately after the \*GASKET BEHAVIOR option.

Abaqus/CAE Usage: Use the first option and any of the following options to specify a gasket behavior:

Property module: material editor:

Other→Gasket→Gasket Thickness Behavior

Other→Gasket→Gasket Transverse Shear Elasticity and/or Gasket

Membrane Elasticity

Mechanical→Expansion

Mechanical→Plasticity→Creep

General→Depvar

General→User Output Variables

<!-- source-page: 947 -->

# Defining the thickness-direction behavior of the gasket

To define the thickness-direction behavior of gaskets, Abaqus/Standard offers a nonlinear elastic model with damage and a nonlinear elastic-plastic model with the possibility of considering creep effects. Thermal effects in the thickness direction can also be accounted for.

Abaqus/Standard measures the thickness-direction deformation as the closure between the bottom and top faces of the gasket element; therefore, the thickness-direction behavior must always be defined in terms of closure. The closure is the sum of the elastic closure, plastic closure, creep closure, thermal closure, plus any initial gap in the thickness direction. As explained below, the behavior can be defined as pressure versus closure, force versus closure, or force per unit length versus closure. In all cases the thickness-direction behavior can be defined as a function of temperature and/or field variables.

Input File Usage: \*GASKET THICKNESS BEHAVIOR, DEPENDENCIES

Abaqus/CAE Usage: Property module: material editor: Other→Gasket→Gasket Thickness Behavior

# Choosing a unit system used to define the thickness-direction behavior

The thickness-direction behavior can be defined in terms of pressure versus closure, force versus closure, or force per unit length versus closure.

Prescribing the thickness-direction behavior as pressure versus closure

You can define the thickness-direction behavior in terms of pressure and closure for all gasket element types. The pressure is available for output or visualization.

Input File Usage: \*GASKET THICKNESS BEHAVIOR, VARIABLE=STRESS

Abaqus/CAE Usage: Property module: material editor: Other→Gasket→Gasket Thickness Behavior: Units: Stress

Prescribing the thickness-direction behavior as force or force per unit length versus closure

You can define the thickness-direction behavior in terms of force or force per unit length and closure only for link elements and three-dimensional line elements. This method is suited for cases where the gasket cross-section in the 1–2 or 1–3 plane varies greatly with deformation because it would be too expensive to model such a deformation with a full two- or three-dimensional model. In such cases a model with link elements or three-dimensional line elements can give meaningful answers as long as the deformation is quantified in terms of force or force per unit length (see Figure 32.6.6–1).

When using two- or three-dimensional link elements, you must specify the thickness-direction behavior as force versus closure. When using axisymmetric link elements or three-dimensional line elements, you must specify the thickness-direction behavior as force per unit length versus closure.

Input File Usage: \*GASKET THICKNESS BEHAVIOR, VARIABLE=FORCE

Abaqus/CAE Usage: Property module: material editor: Other→Gasket→Gasket Thickness Behavior: Units: Force

<!-- source-page: 948 -->

![](images/page-948_798e29bdb29b3e7a92487bd1b039d4c78b2632fce29d8fc9ba8b6cbe1357a191.jpg)

<details>
<summary>text_image</summary>

top block
bottom block
gasket
undeformed configuration
deformed configuration
bottom block
</details>

![](images/page-948_c5b7e6fd9d67e52e6d90219189ef95a032f0d662573fcda3fa34af359a51c5db.jpg)

<details>
<summary>text_image</summary>

force or force per unit load
top block
gasket
element
bottom block
model for analysis
</details>

Figure 32.6.6–1 Modeling complex deformations with link or three-dimensional line elements.

# Defining a nonlinear elastic model with damage

The nonlinear elastic model with damage is illustrated in Figure 32.6.6–2.

![](images/page-948_6c3fa39d8c7f1a837e13fe6508c1d1be3b348566d174c5645ce18ffafa146faf.jpg)

<details>
<summary>line</summary>

| Point | Pressure | Closure |
|-------|----------|---------|
| A     | 0        | A       |
| B     | ~1.0     | C_max_B |
| C     | ~0.5     | C_max_B |
| D     | ~1.5     | C_max_D |
</details>

Figure 32.6.6–2 Elastic model with damage.

<!-- source-page: 949 -->

As the gasket is compressed, the pressure (or force, or force per unit length) follows the path given by the loading curve. If the gasket is unloaded, for example at point B, the pressure follows the unloading curve . Reloading after unloading follows the unloading curve until the loading is such that the closure becomes greater than $C _ { B } ^ { m a x }$ , after which the loading path follows the loading curve . The arrows shown in the figure illustrate the loading/unloading paths of this model.

# Defining the loading curve

To define the loading curve in piecewise linear form, you provide data points of pressure versus elastic closure, starting with point A. For negative elastic closures, the model gives zero pressure (or force). For closures larger than the last user-specified closure, the pressure-closure relationship is extrapolated based on the last slope computed from the user-specified data.

Input File Usage: \*GASKET THICKNESS BEHAVIOR, TYPE=DAMAGE, DIRECTION=LOADING

Abaqus/CAE Usage: Property module: material editor: Other→Gasket→Gasket Thickness Behavior: Type: Damage, Loading

# Defining the unloading curve

To define the unloading curves ( , , and so on), you provide data points of pressure (or force) versus elastic closure up to a given maximum closure $( C _ { B } ^ { m a x }$ , or $C _ { D } ^ { m a x }$ , and so on). You can specify as many unloading curves as are necessary. Each unloading curve always starts at point A, the point of zero pressure for zero elastic closure, since the damaged elasticity model does not allow any permanent deformation. If unloading occurs from a maximum closure for which an unloading curve is not specified, the unloading is interpolated from neighboring unloading curves. The unloading curves are stored in normalized form so that they intersect the loading curve at a unit stress (or unit force) for a unit elastic closure, and the interpolation occurs between these normalized curves. If unloading curves are not specified, the loading/unloading will follow the loading curve.

Input File Usage: \*GASKET THICKNESS BEHAVIOR, TYPE=DAMAGE, DIRECTION=UNLOADING

Abaqus/CAE Usage: Property module: material editor: Other→Gasket→Gasket Thickness Behavior: Type: Damage, Unloading, toggle on Include user-specified unloading curves

# Defining the behavior for elements with an initial gap

For cases when the load in the gasket does not increase as soon as the gasket is compressed (see Figure 32.6.6–3), you can specify an initial gap as part of the gasket section property definition (see “Defining the gasket element’s initial geometry,” Section 32.6.4) and define the loading/unloading curves as if the initial gap were not present (the case of Figure 32.6.6–2). This method is convenient when many gasket elements refer to the same gasket behavior and the only difference is the initial gap.

<!-- source-page: 950 -->

![](images/page-950_18ffc8f70cda964398d9cc128338ed0d20ab7f06d3f5c14f1826fcf3072704bd.jpg)

<details>
<summary>line</summary>

| Point | Curve Type       | Description        |
|-------|------------------|--------------------|
| A     | loading curves   | Initial gap        |
| B     | loading curves   | Initial gap        |
| C     | loading curves   | Initial gap        |
| D     | unloading curves | Initial gap        |
| E     | unloading curves | Initial gap        |
</details>

Figure 32.6.6–3 Elastic model with damage and initial gap.

# Defining a nonlinear elastic-plastic model

The nonlinear elastic-plastic model is illustrated in Figure 32.6.6–4. As the gasket is compressed, the pressure (or force) follows the path given by the loading curve . The loading curve is a nonlinear elastic curve until point B is reached. At point B the slope of the loading curves decreases by more than 10%, which is assumed to correspond with the onset of plastic deformation. The value of 10% was chosen as a reasonable minimum value that can be expected at the onset of yield. If yield starts at a point at which no decrease in the slope occurs, numerical difficulties may occur. If the elastic part of the loading curve has a changing slope, the curve should be defined such that the slope does not decrease by more than 10% at any given point. After point B plastic deformation starts taking place. If unloading occurs before point B is reached, unloading will take place along the initial loading curve. Once loading has gone beyond point B, unloading will take place along an unloading curve such as curve . The unloading is assumed to be entirely elastic. The amount of closure at point D represents the plastic closure for the unloading curve . Reloading after unloading follows the same curve until the gasket yields, after which the loading curve is followed. Plastic deformation takes place until the last point M on the loading curve is reached. Beyond point M, the curve is followed for both loading and unloading; this behavior represents the behavior of a crushed gasket, which is assumed to be entirely elastic and can be specified in a piecewise-linear fashion, even beyond point M. The arrows shown in the figure illustrate the loading/unloading paths for the elastic-plastic model.

Abaqus/Standard will automatically convert the curves so that the unloading curves become curves of pressure (or force) versus elastic closure for a given plastic closure. The loading curve will be transformed into an elastic loading/unloading curve defined at zero plastic closure (the portion of the curve) and a yield curve (the portion of the curve). By default, the onset of yield (point B) will be obtained as soon as the slope of the loading curve decreases by 10% from the maximum slope recorded up to that point while traveling along the loading curve from point A to point M.
