Things to Know Before Building the Model
Some restrictions when using gap and surface contact elements (referred throughout this page as gap elements) in a Static Stress Analysis with Linear Material Models are as follows. Unless noted otherwise, this information pertains to hand-built gap elements, 3D CAD models setup with surface contact, and 2D meshes setup with surface contact.
- Gap elements are not available for linear dynamic analysis.
- The results are independent of the loading history; only the final static result is calculated. Therefore, the loading and unloading do not dissipate the energy due to friction. (In the case of hand-created gap elements, the friction effects between the two surfaces cannot be considered.)
Gap and surface contact elements in a linear stress analysis cause the solution to become an iterative solution. Until the deflections are known, it is unknown which gap elements are opened or closed. Until it is known which gap elements are opened or closed, the deflections cannot be calculated. Thus, the solution method is as follows:
- assume that some of the gap elements are opened or closed on the first iteration
- calculate the deflection
- determine which gap elements are opened or closed and which ones are not
- change the gap element or elements that do not match the assumption
- repeat the analysis until that status of all gap elements is constant
Since it is usually not known how many iterations are required to converge on the solution, the run time for a model with gap elements can be much longer than the same model without gaps.
Stabilizing the Model
One problem that you may need to contend with is rigid body motion in subassemblies that are restrained only by the gap elements. (A subassembly is defined here as any number of parts that are bonded together.) Since the solution is iterative, you always need to be aware of the possibility that some iteration will not include enough gap elements in the solution to provide static stability for all subassemblies. Thus, all parts of the model should 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 restrained with weak springs (weak boundary elements). The goal is to provide stability to all parts, but allow them to move a considerable distance in the process. If gap elements are not part of the solution on some iteration, the weak springs restrain the part so that the processor can calculate a solution, but then the processor detects that some gap elements have come into contact, and then proceeds with the next iteration and includes the gap element. Since the weak boundary elements do not exist in reality, the stiffness needs to be set to have minimum affect on the results.
The details to add the boundary elements are as follows:
- For a subassembly that are restrained partially or solely by the gap elements, select three vertices (Selection
Select Vertices). To provide stability in all directions, the three arbitrary nodes must not be in a straight line. (Fewer than 3 vertices can be used if the subassembly is restrained in some direction by boundary conditions or if the element type is lacking degrees of freedom. The goal of the boundary elements is to make the part statically stable in all six directions: three translations and three rotations.) - Right-click and choose Add Nodal Rigid Boundary.
- Fix the boundary element in X, Y, and Z directions (or as appropriate).
- Enter a value in the Stiffness field. Remember that a boundary element is a spring that connects the node to the ground. Thus, it will transmit part of the applied load to the ground. To minimize the amount of load that is removed from the model, calculate the appropriate stiffness as follows. Estimate the deflection that will occur at the node, and assume some fraction of the applied load will be transmitted through the spring (like 0.1%). The stiffness can be calculated as load/deflection. For example, if the applied load is 1000 lbs and you are willing to let the rigid boundary elements take 1 lb, and if the estimated deflection of the model at the location of the rigid boundaries is 0.05 inches, then an acceptable stiffness would be F/d = (1 lb)/(0.05 inch) = 20 lb/in.
- Click OK to apply the boundary element to the selected vertices.
- Repeat for other subassemblies in the model as needed.
To aid with the stability of the model and the iterative process, review the settings on the Contact tab of the Analysis Parameters. See Contact Options on the page Static Stress with Linear Material Models later in this section.
After the Analysis
After the analysis, review the log file (from the Report environment) to see how the iterative process went. A sample output is below:
| **** Begin solving nonlinear equations | ||||||||
| ITER | CLOSE | OPEN | frON | fOFF | LOADFACT | TOTALf | CLOSED/TOTAL | CRC-CHECK |
| 1 | 9 | 0 | 0 | 0 | 1.0000E+00 | 0 | 9/11 | 123408E4 |
| 2 | 0 | 1 | 0 | 0 | 1.0000E+00 | 0 | 8/11 | 6BB6B604 |
| 3 | 0 | 1 | 0 | 0 | 1.0000E+00 | 0 | 7/11 | 665639D4 |
| 4 | 0 | 1 | 0 | 0 | 1.0000E+00 | 0 | 6/11 | 40CE5738 |
| 5 | 0 | 1 | 0 | 0 | 1.0000E+00 | 0 | 5/11 | FB5D11B9 |
| **** Solution has converged. | ||||||||
where
- ITER is the iteration number. In this sample, 5 iterations were performed.
- CLOSED is the number of gap elements that changed to closed from the previous iteration. In this sample, 9 elements were changed from opened to closed for the first iteration, and then no addition gap elements were closed during any of the remaining iteration.
- OPEN is the number of gap elements that changed to opened from the previous iteration. In this sample, one element was opened for each iteration 2 through 5.
- frON and fOFF are the number of gap elements that changed from the previous iteration to include friction or to remove friction, respectively.
- LOADFACT is the load factor applied to the model.
- TOTALf is the total number of gap elements with friction.
- CLOSED/TOTAL is the number of gap elements that are closed out of the total number of gap elements in the model.
- CRC-CHECK is a way for the processor to detect that the solution is oscillating. Two iterations have the same status for all the gap elements. If it proceeds, the processor repeats the same iteration cycle indefinitely. When such oscillations are detected, the solution stops, and the log file contains a message about the solution being quasi-periodic.
- Solution has converged indicates that a successful solution was obtained. Other messages are Solution has not converged after n iteration and A quasi-periodic solution achieved. The periodic solution indicates that two different iterations found the same set of gap elements were opened and closed. Your system may lack stability for the processor to find the static solution; in this case, try adding boundary elements. The second option is to adjust the contact parameters on the Analysis Parameters dialog.
If boundary elements were used to stabilize any parts of the model, use the Results environment to check the axial force in the boundary elements. The amount of axial force should be insignificant compared to the applied loads in the model.