Featured Case StudyThe Norsea Gas Terminal in Northern Germany plays a vital role in the connection of pipeline systems coming from the North Sea to the natural gas distribution network throughout Germany. Built in...Stay
- ANSYS Software
Featured Case StudyRelying on ANSYS Composite PrepPost helped EADS Innovation Works to develop lightweight composites in aircraft design. ANSYS Composite PrepPost provided simple pre- and post-processing of composite...Stay
- Resource Library
- News &
How Can I Get My Contact Problem to Converge?
How many times have you set up a contact analysis only to find that it won’t converge? Maybe you even tried adding a lot of substeps to ramp on the load slowly, or perhaps you tried some of the suggestions included in my colleague Peter Barrett’s excellent blog "Stress Analysis Convergence Tips for “Dummies”". This blog includes some important background about nonlinear analysis and convergence, and discusses different methods for overcoming convergence problems. Relating to contact analysis specifically, it proposes the following methods:
1. Fix the Rigid Body Motion:
a. Start with all parts in the assembly touching. This can be achieved by moving bodies, adding contact offsets, or adding stabilization damping.
b. Add friction to the contact surfaces.
2. Overcome Non-Convergence:
a. Reduce the stiffness of the contact elements. (My experience has shown that ramping loads slowly and/or lowering contact stiffness will solve 90% of convergence issues).
b. Refine the mesh in the contact region to reduce the percentage of elements flipping in and out of contact.
In this article, I’m going to use a specific example to demonstrate some of the above methods and also describe several other methods to help overcome stubborn contact-related convergence problems. It is important to note that many FEA codes, like ANSYS, have heuristics built in that attempt to set program defaults in order to achieve fast convergence and an accurate solution. However, it is impossible to devise these heuristics so that they work automatically for every single contact condition. They are designed to address the common situations, but may need manual intervention for some cases.
In this example, a plate spring is compressed by a flat rigid plate subjected to an applied force as shown in Figure 1. (Shown above) The ANSYS finite element code was used for this analysis. Several attempts were required to obtain a converged solution.
The first attempt at a solution did not converge, giving the following error: “An internal solution magnitude limit was exceeded”. This type of error, and others such as “Small negative equation solver pivot term” or simply “Solver pivot warnings or errors have been encountered”, is indicative of rigid body motion. In fact, the unconverged solution shows that the rigid plate passed right through the top of the spring (Figure 2)!
Figure 2: Unconverged Solution Showing Rigid Body Motion in the Compression Plate
Close inspection of the geometry shows an initial gap between the contact surfaces (Figure 3).
Figure 3: Initial Gap at the Contact Pair
Finite element codes such as ANSYS can provide diagnostic information about the initial contact status including the minimum gap or maximum penetration, such as the information shown below for this example:
Had I looked at this information before I ran the model, I would have easily avoided this problem.
Problem: Initial gap between contact parts with no constraints to prevent rigid body motion.
Solution: Close the initial gap.
The initial gap can be closed either by moving the parts together until they are just touching or by applying a numerical offset to the contact surface. ANSYS provides a contact offset value that can be entered manually or can be automatically calculated to provide an “Adjust to Touch” configuration. In this attempt, the “Adjust to Touch” option was used to close the gap.
Unfortunately, this 2nd attempt also failed to converge after numerous iterations and bisections. Once again, the error message is “An internal solution magnitude limit was exceeded”, indicating rigid body motion. But why would rigid body motion occur if the contact gap was closed? This can sometimes happen when too much load is applied to the contact interface in one step, causing the contact surfaces to separate or over-penetrate. In this case, all of the load was applied in one step. In addition, the plate spring is a very flexible structure. Default contact stiffnesses are usually too high for contact involving highly-flexible structures, causing the contact surfaces to separate.
Problem: Load applied in one step and contact stiffness probably too high.
Solution: Use multiple substeps to ramp on the load more slowly and reduce the contact stiffness.
In this attempt, additional substeps were added to apply the load more slowly. The contact stiffness was also reduced and an option was selected to let the solver adjust the stiffness throughout the nonlinear solution, as needed to improve convergence behavior.
This attempt converged quickly, resulting in the displaced shape shown in Figure 4.
Figure 4: Final Deflected Shape
Contact penetration was checked to confirm that the reduced contact stiffness did not result in over-penetration. Problem solved!
In hindsight, convergence could have been achieved on the first attempt by:
a. Checking the gaps.
b. Applying the load slowly.
c. Lowering the contact stiffness to account for the high geometric flexibility of the spring.
Other methods to Improve Convergence Behavior:
Unfortunately, real-world models involving contact between multiple parts are not always as simple as our example and other methods might be needed to obtain convergence. Here are some additional recommendations:
Plot Residual Forces: High values of the Newton-Raphson residual forces typically indicate the specific contact pair(s) that are causing the non-convergence.
Refine the mesh in the contact zone: This will distribute the contact pressure over more elements and increase the number of points in contact. Relatively few points in contact can cause very high contact stresses, resulting in excessive element distortion and convergence difficulties. This is particularly a problem with nonlinear materials.
Use Surface Projection Based Contact (AKA – Detection Method = Nodal-Projected Normal from Contact in ANSYS): This method generally improves the distribution of contact pressure and traction, especially when the meshes on the mating contact surfaces are significantly different. It also tends to provide a more accurate stress solution in the underlying elements.
Add Contact Stabilization Damping: This is another method you can use to eliminate rigid body motion in cases where there is an initial gap between bodies. This provides an alternative to manually moving the bodies into contact, adding an offset, or using an “adjust-to-touch” option. While those methods are effective, they can alter the perceived geometry by effectively offsetting the location of the contact detection points. Contact stabilization damping, on the other hand, damps out relative motion between the parts, allowing the parts to move relative to each other and close the gap.
The example I presented in this article provides a typical process used by an analyst to obtain a converged solution to a contact problem. The model contained some problematic features common to contact models. I highly recommend that you also review the presentation “ANSYS Nonlinear Convergence Best Practices” for more helpful recommendations.
Please let us know of any experiences you’ve had in getting your difficult contact models to converge. What caused the convergence problems and how did you overcome them?
by: Chris Mesibov
by: Chris Mesibov
by: Chris Mesibov
by: Chris Mesibov
by: Peter Barrett
- Engineering Consulting
- ANSYS Software & Support
- ANSYS Training
- About Us
- News & Insights
1579 Straits Turnpike Suite 2B
Middlebury, CT 06762
- ANSYS Software