Defining the gasket element's initial geometry

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.

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.

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

GASKET SECTION
thickness

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

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.

GASKET SECTION
 , , , additional geometric data (cross-sectional area, width, or out-of-plane thickness)

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

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 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.

Figure 1. Thickness direction for a link element.

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 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.

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

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 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.

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

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 4).

Figure 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.

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

GASKET SECTION
 , , , , component 1, component 2, component 3

NORMAL

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) 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.

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.