Assembly + contact - apply loads, contacts penetrate too far.... 2

[coteesh]

I am constantly having problems making assemblies with contact elements converge. I am aware of the various types of contacts and the differences between them (pure penalty, Lagrange, etc) and that symmetric formulation is more reliable when targets and contacts are not clear. I often must simulate 2D axisymetric as well as 3D assemblies where one part of the assembly is fixed, and another part has a load or torque applied directly to the assembly. Often a dozen or more parts all in contact. I run the solution as small displacement static nonlinear with automatic time stepping in ANSYS Classic and the "initial penetration" of the elements is always too large and quite often the problem will never converge, and the contacts have gone right through each other. Do I need to apply some kind of "ramped" load to the assembly instead of the full load all at once?


I have also tried using Workbench, and with the weak-springs option turned on. I have very limited success and run into the same problems as above and problems won't converge. The assembly is properly constrained to prevent items from oving off to infinity with "rough" contacts, etc.

I'm aware that some contact elements are better than others. I have followed some suggestions in this PDF file:

http://www.midwest-ansys-ug.com/051805_presentations/051805_maug_contact_presentation.pdf

"automated adjustment of initial contact conditions"

with almost no success.

Does anyone have any good solid tips so that my problems will converge better and prevent initial penetration? In particular I am using Ansys Workbench for large 3D assemblies (I'm mad that there are no P-elements but that's a different story) and Ansys Classic mainly for 2D.

Thanks.

 

[cbrn]

Hi,
surface / surface contacts can be very hard to converge if the surfaces in contact experience high "rotation" one with respect to the other, i.e. if the contact tends to become "edge - over - surface".
In these cases, it is recommended to lower the contact stiffness and/or to increase the contact penetration allowance.
Most often I obtained good results by lowering the contact stiffness and maintaining the "default" penetration, all this with the update of contact stiffness at each equilibrium iteration (this last, in my opinion, is a very important point): at first, the penetration won't be respected, but the iteration will converge: in this case, you will have a solver message saying "XXX points have too much penetration", and subsequently more iterations will be performed even if the force norm / displacement norm have converged.
If you see that more time is needed to respect the penetration than to converge the equilibrium iteration, then it is the signal that your mix of stiffness / penetration is unbalanced (too strict a penetration / too low a stiffness; but if you increase stiffness you may return to convergence problems...).
In all these cases, I would never let the program perform bissections automatically, since you can run into infinite solution times (Ansys trying to get smaller and smaller time steps in order to obtain convergence): it is better, IMO, to see the solution diverge and stop it in order to make some changes in the settings.
IMExp, a properly set contact problem should converge in max 20 equilibrium iterations; inside each of them, with PCG solver you shouldn't overcome 1000 iterations.

Which brings me to another important point: in case of "difficult" contact problems, SPARSE SOLVER is enormously more efficient (and is recommended by ANSYS itself - see help). In this case, you may find this command helpful:
BCSOPTION,,<solution logic>,<mem size>,,,<diagnostics>

Hope this helps...

Regards