Contact problem convergence - debug tips

[maheshh]

All

I have been having convergence issues with a contact problem that I have set up. Can somebody give me generic pointers in how to go about debugging why the problem is not converging?

To give a very generic backgrouund - I have a steel component which has a remote displacement boundary condition and it pressing on another steel component. Because of this interaction, there are other components which have contacts (at first step, or come in contact at a later time step).

In all I have about 2 bonded/no-seperation, 3 frictionless contacts.

The force convergence always looks similar to the attached picture.

Any help is appreciated.

Thanks in advance.

 

[fuzzdoug]

from the screen shot it appears you are using workbench...

these are some steps i use to troubleshoot assemblies.

1. Turn on "Newton-Raphson Residuals" under Solution Information. Enter in 3-4 for the value for the number of previous iterations. This will allow you to plot areas where force equilibrium are a possible problem. This will at least give you an idea if the problem areas are the interaction of parts. (which is most of the time for me.)

2. It's possible you could be getting "chattering" between contacts. This could be alleviated by adjusting your contact stiffness. Maybe the contacts are "too stiff" to properly converge. Just keep in mind you'll could be sacrificing accuracy due to excessive penetration. Try a value of .01-.001 for "Normal Stiffness" under the Advanced Features of your contacts.

3. Adjust your time steps. Use smaller increments.

4. Your mesh could also not be refined enough in contact areas.

5. Readup on the Results Tracker.

 

[fuzzdoug]

is there no edit feature for threads?

anyway...
i just took a look in the ansys help file for workbench and found some good guidelines:

Simulation Help -> Troubleshooting -> Problem Situations -> The Solver Engine was Unable to Converge

 

[Stringmaker]

In this case I'm not certain that I believe your problem is with the actual contact. It seems that you may have conflicting constraints of some type which cause a sort of singularity. As dmangels suggested above, the NR residual plots should tell the story. You'll probably find one or two spots in your model that have high residual forces with the rest of it being well converged.

Good luck.