How to Perform Linear Contact Analysis with Linear Gap Elements

ALGOR software provides extensive capabilities for multiple-body contact and interaction. Among these capabilities, contact between parts during a linear static stress analysis can be modeled using linear gap elements. This technique is most often used for hand-built models, but can also be used for CAD assemblies.

A linear gap element is used when:

• You wish to model the effects of a spring (compression only) or cable (tension only) where the stiffness is not always present under all loadings.
• You wish to know the contact force between two parts under load.

In a linear stress analysis, gap elements force the solution to become an iterative process. Until the deflections are calculated, it is not known which gap elements are in contact. Until it is known which gap elements are in contact, the deflections cannot be calculated. Thus, the solution method is as follows:

• determine which of the gap elements are in contact on the first iteration
• calculate the deflection
• determine which gap elements would have come into contact
• add those elements to the solution
• repeat the process until the status of all elements is constant

The important thing to keep in mind is that the gap elements may not contribute to the solution on the first iteration or any subsequent iteration. Thus, all parts of the model must be statically stable without relying on the gap elements.

In cases where parts are "free" to move until they interact with other parts, these free parts must be constrained with weak springs (boundary elements, which allow for a flexible connection between a finite element model and fixed points in space). The goal is to provide stability to all parts, but allow them to move a considerable distance in the process. After the first iteration, the analysis processor detects that some gap elements have come into contact, and then proceeds with the next iteration and includes the gap elements.

Consider the example shown in Figures 1-3, which illustrate this procedure.

Figure 1: In a hand-built model, two aluminum blocks (the green elements) will come into contact during the analysis. The top block is constrained from translation in the Y direction and is loaded with an applied pressure on its top surface. The bottom block is fixed on its bottom surface. Linear gap elements (the red lines) are defined between the nodes of the blocks where contact will occur. Arbitrarily, two nodes of the top block are selected (highlighted by magenta dots) and elastic boundary elements are added in the FEA Editor environment.

Figure 2: The stiffness of the elastic boundary elements is set to a low value, where "low" depends on the units and the amount of force to be carried by the boundary elements.

Figure 3: The weak elastic boundary elements will provide sufficient stiffness in the Z direction during the iterations of the solution to ensure stability of the model. During the analysis, the linear gap elements will come into contact.

This example required constraints in only one direction (Z) for stability. For parts that require constraints in multiple directions to provide stability, use multiple boundary elements (one for each direction).

For more information about linear gap elements and multiple-body contact and interaction, see the ALGOR User's Guide.