Gaskets are widely used in many assemblies and play essential roles in sealing and transferring force. While some gaskets have simple geometry and material components, most are made of complicated structure and material components. They exhibit complicated and highly nonlinear behavior under compressive loading and unloading. It is usually not practical to model gaskets according to their exact geometry and material components. In reality, it is the mechanical response of gaskets that matters most. Therefore, a special gasket element can be designated to simulate the gasket behavior and to avoid fine details of gasket itself.
The gasket element behavior is unique in the following areas:
- Only compressive stresses through the thickness are developed and transmitted. Stresses and forces in the plane of the gasket are ignored. So even though the gasket part may be bonded to the mating part (by virtue of using the same nodes on each part), the connection is better thought of as a 0 friction surface since no shear forces are developed in the gasket.
- The mesh must be created with just one element through the thickness.
- In some situations, the user needs to indicate which surfaces are the top and the bottom. This occurs when the thickness dimension (in the compression direction) of the gasket is larger than the width (normal to the compression direction). See below.
- The material properties are specific to a given thickness of gasket.
3D gasket elements can have these geometric forms: bricks (8 corner nodes, 6 quadrilateral sides), wedges (6 corner nodes, 2 triangular sides, 3 quadrilateral sides), pyramids (5 corner nodes, 4 triangular sides, 1 quadrilateral side), and tetrahedral (4 corner nodes, 4 triangular sides). Since only one element is permitted through the thickness, at least one of the faces of the tetrahedral element must be on the top or bottom of the gasket.
The material model of the gasket element includes the capability of a multi-linear elastic curve, a yield point, multi-linear plastic curve, and multiple unloading curves, each of which is defined by multi-linear curves.
Apply Loads to Surfaces
Uniform pressure, traction, and hydrostatic pressure can be applied only to the top face or bottom face of the 3D gasket element, but not to both.
If the model originated from a CAD solid model and has not been altered manually, the pressure can be applied by selecting the surface of the face where the pressure is appropriate. The surface numbers of the individual lines making the face are not critical. A pure CAD model knows what faces belong to the surface. The pressure will be applied if the selected surface is the top or bottom face of the gasket.
For parts that were meshed by hand, or if the CAD model was altered (and therefore you are working with the equivalent of a hand meshed model), the lines making up the face of the element need to have a majority of the lines on the same surface number in order for the pressure to be applied to the face. For a four node face, any three of the four lines on the same surface number determines the surface number of that face. For a three node face, any two of the three lines on the same surface number determines the surface number of that face, Then, the highest surface number among the faces that define the 3D gasket element determines the surface number of the element. The pressure will be applied if the selected surface is the top or bottom face of the gasket.
Basic Steps for Use of 3D Gasket Elements
- Be sure that a unit system is defined.
- Be sure that the model is using a nonlinear analysis type.
- When creating the mesh of the gasket, use one element through the thickness. Note that the mesher for CAD solid models has a special setting for creating a mesh with one element. (See Meshing CAD Solid Models)
- Right-click the Element Type heading for the part that you want to be 3D gasket elements.
- Select the 3D Gasket command.
- Right-click the Element Definition heading.
- Select the Edit Element Definition command.
- Specify the appropriate input in the Element Definition dialog to specify the solution parameters for the gasket element.
- Press the OK button.
- Right-click the Material heading for the part and choose Edit Material. Enter the material properties for the gasket.
- Select the surface or surfaces that define the top face and bottom face of the gasket. This can be done in the display area (Selection Select Surfaces) or in the Surfaces branch of the tree view. (The two faces can be on the same surface number or different surface numbers.) Right-click and choose Gasket's Top/Bottom Surface. When working with a hand-built mesh, the lines on the sides of the gasket that connect the top and bottom faces should not be on the same surface number as the top or bottom surface.
Advanced 3D Gasket Element Parameters
The other parameters on the Element Definition dialog determine the behavior of the gasket during the analysis.
- Analysis Formulation pull-down determines if large deflection effects are included in the analysis. If Geometrically nonlinear is chosen, the changing thickness and orientation of the gasket is based on the current gasket deformation. Large deflection effects due to geometry changes are included. If Linear is chosen, the thickness and orientation are calculated from the original position. Small deflections effects are assumed and effects due to the geometry changes are ignored.
- Integration Order pull-down sets the accuracy of the calculation across the element. For rectangular shaped elements, select the 2nd Order option. For moderately distorted elements, select the 3rd Order option. For extremely distorted elements, select the 4th Order option. The computation time for element stiffness formulation increases as the third power of the integration order. Consequently, the lowest integration order which produces acceptable results should be used to reduce processing time.
- Stabilization Factor field provides numerical stability for models. Since the gasket only has stiffness in the thickness direction, motion perpendicular to the thickness can be unstable, especially if performing a static stress analysis and if the parts connected through the gasket are not restrained by other means (bolts connecting the parts, boundary conditions, and so on). The Stabilization Factor can be zero when the gasket is well constrained. The stiffness added by the Stabilization Factor is the product of the stabilization factor and the stiffness of the last segment of the gasket material property curve. Since this is added stiffness to the diagonal terms of the elasticity matrix, it should be sufficiently small so that it will not affect the convergence and accuracy of the results.
- Use default initial thickness direction throughout check box is available only if the Analysis Formulation is set to Linear. When activated, the thickness of the gasket is set to a constant thickness specified by the Scalar X, Scalar Y, and Scalar Z inputs. This can be beneficial for very thin gaskets where the numerical error in the nodal coordinates can have a significant effect on the thickness.