<!-- source-page: 931 -->

# Discretizing a gasket with gasket elements that model thickness-direction behavior only

When discretizing a gasket with several layers of gasket elements along the gasket direction, it is recommended that all the nodes belonging to a cross-section of the gasket have the same thickness direction (see Figure 32.6.3–4). An approximate solution will be generated if the thickness direction changes, since only the magnitude of the force is transmitted from one gasket element to the next through the thickness of the gasket.

![](images/page-931_35b239d869b460ae7e6456f30a40bf015bf7c84b010476d8e22fc97a79b15c56.jpg)

<details>
<summary>text_image</summary>

n
n
n
n
cross
section
</details>

Figure 32.6.3–4 Discretizing a gasket using several layers of elements with thickness-direction behavior only.

# Connecting gaskets to other components when gasket elements with thickness-direction behavior only are chosen

Contact pairs can be used to connect the gasket mesh to adjacent components, as explained above, but only frictionless, small-sliding contact can be used.

MPC type PIN or TIE can also be used to connect a one degree of freedom node of a gasket element to another coincident node that has all its displacement degrees of freedom active (see Figure 32.6.3–5). Abaqus/Standard automatically constrains the single displacement degree of freedom node to the global displacements of the other node.

Surface-based tie constraints cannot be used to connect gasket elements that model thickness-direction behavior only.

# Additional considerations when using gasket elements

Several cases require special consideration when using gasket elements.

<!-- source-page: 932 -->

![](images/page-932_ee104940b1573fe806397fa6f37a45a0408903836d6a8967c647300d8ee5c063.jpg)

<details>
<summary>flowchart</summary>

```mermaid
graph TD
    A["part 1"] --> B["gasket elements"]
    B --> C["part 2"]
    C --> D["coincident node"]
    D --> E["1 d.o.f."]
    E --> F["Use TIE- or PIN-type MPC"]
    F --> G["2 d.o.f."]
```
</details>

Figure 32.6.3–5 Connecting gasket elements with thickness-direction behavior only to other parts by using MPCs.

# Using gasket elements in large-displacement analyses

Gasket elements are small-strain, small-displacement elements. They can be used in large-displacement analyses. However, the local directions of the gasket elements are not updated with the solution, so incorrect results will be generated if the assembly containing the gasket elements undergoes any significant amount of rotation.

# Using 12-node gasket elements

These elements are primarily for use when the adjacent components are modeled with modified 10-node tetrahedral elements (element type C3D10M). When the contact pair approach is used, such elements can also be placed adjacent to other three-dimensional solid continuum elements; however, if the meshes are badly mismatched, the solution may be noisy.

# Using 18-node gasket elements

These elements are intended to share nodes with 21 to 27-node brick elements. They can also be connected to a mesh composed of 21 to 27-node brick elements or a mesh composed of 20-node brick elements when the contact pair approach is used.

Abaqus/Standard allows the node numbers and the coordinates of the midface nodes in the 18-node gasket elements to be generated automatically if the faces are part of contact surfaces, similar to the way that midface nodes are generated for 20-node brick element faces on which a contact surface is defined. This feature is invoked by leaving the entries for nodes 17 and 18 in the element connectivity blank.

<!-- source-page: 933 -->

# Using the three-dimensional line gasket elements

Three-dimensional line gasket elements are typically used to model narrow, thicker features in gaskets, such as an elastomeric insert around a hole. A typical mesh for such a case is presented in Figure 32.6.3–6. The gasket is discretized mainly with three-dimensional area elements. The insert is modeled with three-dimensional line elements that may or may not be connected to the area elements. These gasket elements are connected to surrounding components using two sets of contact pairs, and the area elements will typically have initial gaps specified in the gasket property definition so that the thicker inserts develop pressure on contact before the area elements do.

![](images/page-933_19d8652a5a08d5453a8576e86a392ed8fbbf3e00e7138304835675f103d7aaf8.jpg)

<details>
<summary>text_image</summary>

nodes of the line gasket elements
area gasket elements
three-dimensional line gasket elements
</details>

Figure 32.6.3–6 Typical use of three-dimensional line gasket elements to model inserts in gaskets.

If three-dimensional line gasket elements that have all displacement degrees of freedom active at their nodes are used to discretize a gasket and the local 3-direction is the same at all the nodes of these elements (this is the case when all elements lie in a plane), the nodes of these elements can move in the local 3-direction without creating any strain in the elements (see “Defining the gasket behavior directly using a gasket behavior model,” Section 32.6.6, for additional details about the local direction of threedimensional line elements). In such a case you should make sure that these elements are restrained properly in the local 3-direction.

<!-- source-page: 934 -->

<!-- source-page: 935 -->

# 32.6.4 DEFINING THE GASKET ELEMENT’S INITIAL GEOMETRY

Products: Abaqus/Standard Abaqus/CAE

# References

• “Gasket elements: overview,” Section 32.6.1   
• \*GASKET SECTION   
• “Creating gasket sections,” Section 12.13.15 of the Abaqus/CAE User’s Guide, in the HTML version of this guide

# Overview

The initial gasket geometry:

• is defined by the nodal coordinates of the element; and   
• is also defined by the thickness direction and initial thickness, each of which can be calculated by Abaqus/Standard or user-defined.

# Defining the element geometry

A gasket element is basically composed of two surfaces (a bottom and a top surface) separated by the gasket thickness. The element has nodes on its bottom face and corresponding nodes on its top face. Two methods are available to define the element geometry.

# By defining the element’s nodes

You can define the geometry of the gasket element by defining the coordinates of all the element’s nodes. You can define elements with constant or varying thickness. If the gasket element is very thin in comparison to dimensions in its surfaces, the thickness of the element calculated from the nodal coordinates may be inaccurate. In this case you can specify a constant thickness directly.

# By defining the bottom surface of the element

You can specify a list of only the nodes on the bottom surface of the gasket element and the positive offset number that will be used to define the corresponding nodes on the top surface of the gasket element. Abaqus/Standard will create the nodes of the top face coincident with those of the bottom face unless the nodes of the top face have already been assigned coordinates. If the bottom and top nodes coincide, you must specify the thickness of the gasket element.

# Specifying the element thickness

You can specify the gasket element thickness as part of its section property definition.

Input File Usage: \*GASKET SECTION thickness

<!-- source-page: 936 -->

Abaqus/CAE Usage: Property module: Create Section: select Other as the section Category and Gasket as the section Type: Initial thickness: Specify: thickness

# Additional quantities needed to specify the element geometry

For three-dimensional area elements, the element geometry is defined entirely by the location of the top and bottom surfaces and the element thickness. For two- and three-dimensional link elements (elements with two nodes, one on each face) you should specify the cross-sectional area of the element. For axisymmetric link elements you should specify the width of the element. For general two-dimensional elements the out-of-plane thickness is required. For three-dimensional line elements you should also specify the width of the element. This additional information is specified as part of the gasket section property definition; if it is not specified but is needed, it is assumed to have a value of 1.0.

Input File Usage: \*GASKET SECTION , , , additional geometric data (cross-sectional area, width, or out-of-plane thickness)

Abaqus/CAE Usage: Property module: Create Section: select Other as the section Category and Gasket as the section Type: Cross-sectional area, width, or out-of-plane thickness: additional geometric data

# Default element thickness-direction definition

Gaskets are usually manufactured to have a desired behavior in their thickness direction. Therefore, it is important to define the thickness directions of gasket elements accurately. Abaqus/Standard computes these directions by default. The method that Abaqus/Standard uses depends on the gasket element type.

# Link elements

Abaqus/Standard computes the thickness direction for a two-dimensional, three-dimensional, or axisymmetric link element by subtracting the coordinates of node 1 from those of node 2, as shown in Figure 32.6.4–1. The computed thickness direction is then assigned to each node. If the gasket element is very thin, the thickness direction may not be predicted accurately. You can overwrite this direction, as explained below in “Specifying the thickness direction explicitly.”

# Two-dimensional and axisymmetric elements

To compute the thickness direction for two-dimensional and axisymmetric elements, Abaqus/Standard forms a midsurface by averaging the coordinates of the node pairs forming the bottom and top surfaces of the element. This midsurface passes through the integration points of the element, as shown in Figure 32.6.4–2. For each integration point Abaqus/Standard computes a tangent whose direction is defined by the sequence of nodes given on the bottom and top surfaces. The thickness direction is then obtained as the cross product of the out-of-plane and tangent directions. The thickness direction computed at each integration point is then assigned to the nodes on either side of the integration point.

<!-- source-page: 937 -->

![](images/page-937_49deea3d890a434ac13f6d4d8769c84b1617ca0a4d011e2ff555e82884367c42.jpg)

<details>
<summary>text_image</summary>

1
2
n
n
n
</details>

Figure 32.6.4–1 Thickness direction for a link element.

![](images/page-937_71b8007b2e6145b125b176751e2886135be5439edcc1f056ee03c9bc38c48fd0.jpg)

<details>
<summary>text_image</summary>

midsurface
n₁ 4
n₁ 5
n₂
6
n₃
t₁
n₂
t₂
n₁
1
2
3
n₃
t₃
</details>

Figure 32.6.4–2 Thickness direction for a two-dimensional or axisymmetric element.

# Three-dimensional area elements

To compute the thickness direction for three-dimensional area elements, Abaqus/Standard forms a midsurface by averaging the coordinates of the node pairs forming the bottom and top surfaces of the element. This midsurface passes through the integration points of the element, as shown in Figure 32.6.4–3. Abaqus/Standard computes the thickness direction to the midsurface at each integration point; the positive direction is obtained with the right-hand rule going around the nodes of the element on the bottom or top surface. The thickness direction computed at each integration point is assigned to the nodes on either side of the integration point.

# Three-dimensional line elements

To compute the thickness direction for three-dimensional line elements, Abaqus/Standard computes the thickness direction at each integration point of the line element by differencing the coordinates of the element’s surface nodes associated with the integration point. The thickness direction will point from the node on the bottom face to the node on the top face of the element. The thickness direction computed at each integration point is then assigned to the nodes on either side of the integration point (see Figure 32.6.4–4).

<!-- source-page: 938 -->

![](images/page-938_94f441b8b759ea2937c9cf125e82c6af9b79f58be722c13db70d824fa5d73ab7.jpg)

<details>
<summary>text_image</summary>

n₁
5
n₁
n₁
1
n₄
8
n₄
n₄
n₄
n₃
7
n₃
n₃
n₂
6
n₂
4
n₂
2
3
midsurface
</details>

Figure 32.6.4–3 Thickness direction for a three-dimensional area element.

![](images/page-938_a6df06ee568c9266231f77e9f36adf1553bd19c468d607f13c889375289ba71a.jpg)

<details>
<summary>flowchart</summary>

```mermaid
graph TD
    1 -->|n1| 4
    1 -->|n2| 5
    2 -->|n2| 6
    3 -->|n3| 6
    4 -->|n1| 5
    5 -->|n2| 6
    6 -->|n3| 3
```
</details>

Figure 32.6.4–4 Thickness direction for a three-dimensional line element.

If the gasket element is very thin, the computation of the thickness direction may not be accurate. You can overwrite this definition as explained below in “Specifying the thickness direction explicitly.”

# Creating a smooth gasket

Gasket elements can be used in a single layer or can be stacked in multiple layers (see “Including gasket elements in a model,” Section 32.6.3, for further details). The thickness directions computed at the nodes of gasket elements on an element-by-element basis are averaged at nodes shared by two or more gasket elements. This averaging process ensures that, if the gasket is not planar, it has a thickness direction that varies smoothly even though the gasket has been discretized by elements. You must ensure that the connectivities of the elements are such that the thickness direction does not reverse from one element to the next for this process to work properly. Once the averaging process is complete, the thickness directions at the nodes of a given element may vary significantly along the gasket midsurface and through

<!-- source-page: 939 -->

its thickness, as shown in Figure 32.6.4–5. The thickness directions at any of the nodes of an element should not vary in direction by more than 20°. In addition, the thickness directions of two associated nodes through the thickness direction should not vary in direction by more than 5°. Abaqus/Standard will require that the gasket be remeshed when such conditions are not met.

![](images/page-939_a4e97919e447016a61a17dc7ff775bf759379b100fb5a6a4c465913c1653809b.jpg)

<details>
<summary>text_image</summary>

multi-layered
gasket
thickness
direction
20°
5°
3
4
1
2
midsurface
</details>

Figure 32.6.4–5 Result of the averaging process.

# Specifying the thickness direction explicitly

For cases when the above averaging process is not satisfactory, two methods are provided to specify the thickness direction of gasket elements.

Specifying the thickness direction as part of the gasket section definition

You can specify the components of the thickness direction as part of the gasket section definition. In this case all nodes of the gasket elements using this section definition are assigned the same thickness direction. The thickness direction specified at the nodes of the element will be averaged at nodes shared by two or more elements.

Input File Usage: \*GASKET SECTION

, , , , component 1, component 2, component 3

Abaqus/CAE Usage: You cannot specify the gasket thickness direction in Abaqus/CAE.

Specifying the thickness direction by specifying a normal direction at the nodes

You can define the thickness direction at a particular integration point of a gasket element by specifying a normal direction for the node on the bottom face of the element that is associated with the integration point (see “Normal definitions at nodes,” Section 2.1.4). The thickness direction will not be averaged if

<!-- source-page: 940 -->

this node belongs to more than one element. The thickness direction specified at the bottom node will also be assigned at the top node associated with the same integration point. This thickness direction will not be averaged if the top node belongs to more than one element; however, you can overwrite this thickness direction by specifying a normal at this node if it is the bottom node of another element. This last situation can occur only in cases when gasket elements are stacked up through the thickness direction of the gasket. If this method is used to specify conflicting thickness directions at the same node, Abaqus/Standard will issue an error message. Thickness directions specified using this method will overwrite any thickness directions specified at a gasket node as part of the gasket section definition.

Input File Usage: \*NORMAL

Abaqus/CAE Usage: User-specified nodal normals are not supported in Abaqus/CAE.

# Creating fold lines

It is possible to introduce a fold line in a gasket by creating gaskets with coincident nodes and using MPC type TIE or PIN (“General multi-point constraints,” Section 35.2.2) to constrain the displacement of these nodes. However, fold lines are rarely needed in the analysis of gaskets, since almost all gaskets are manufactured with smoothly varying surfaces.

# Verifying the thickness direction

Thickness direction definitions can be checked by examining the analysis input file processor output. The direction cosines of the thickness directions obtained at the nodes of gasket elements are listed under GASKET THICKNESS DIRECTIONS in the data (.dat) file.

# Specifying an initial gap and an initial void in the thickness direction of a gasket element

The construction of gaskets in their through-thickness direction may be complex; for example, certain automotive gaskets are usually composed of several layers of metal and/or elastomeric inserts, and it is likely that the layers do not all touch until the gasket is compressed. The inter-layer spaces in a gasket are referred to in Abaqus as the initial void. The initial void is used only for calculating thermal strain and creep strain. It is also possible that the gasket surface geometry is such that pressure will not start building up until the gasket has been compressed by a certain amount. The gasket closure that is needed to generate a pressure is referred to in Abaqus as the initial gap. Figure 32.6.4–6 shows a schematic representation of the initial gap and initial void in a typical gasket. You can specify both the initial gap and initial void as part of the gasket section property definition. The initial thickness of the element should include the initial gap and the initial void.

Input File Usage: \*GASKET SECTION

, initial gap, initial void

Abaqus/CAE Usage: Property module: Create Section: select Other as the section Category and

Gasket as the section Type: Initial gap: initial gap, Initial void: initial void
