Rigid to flexible surface contact

[mon1299]

Hi everyone,
I am doing nonlinear analysis of a beam rested on a support. I modeled the beam with shell181 element and the support as an area.I define Rigid to flexible contact between the support and the beam where the support is rigid and beam surface as flexible. Time=1, and substep=40. I am wondering when I stop the solution and restart again from the last converged solution, the solution fails to converge and says: too much penetration at some points. I think these message means contact failure. If I continue the solution without stop and restart,I am getting the converged solution for the same model. I cant understand why this thing is happening? Is there anyone who can explain it? I really need your help and comments in ths regards.
Thanks
Mon

 

[Stringmaker]

Mon, I'm a little confused with the problem and whether you're happy with the current outcome or not. Too much penetration is common if you have large changes in contact force and/or pressure between substeps. Ansys is usually pretty good at resolving this. But at any rate I can offer you two suggestions.

1) Make sure you're using the Augmented Langrange contact algorithm (keyop2 = 0)
2) Try changing your contact detection to nodes from Gauss points (keyop4 = 1)
3) Update contact stiffness every equilibrium interation (keyop10 = 5)

If you could give a little bit more of a case by case explanation that would help me out. Sorry my slowness is a sure indication I've been working with Ansys too much. My mind has gone numb.

Hopefully this helps!

-Brian

 

[mon1299]

Hi Brian,
Thanks for your reply.I wanna explain my problem a little bit more:
For my analysis I am using 40 substeps and got good results. I am ok with that.I am writing results for every substep. If I stop the analysis suppose after 20 substeps and then restart the solution from the last substep, the solution can not converge any more due to contact failure. I am using exactly the same condition for both cases.It seems something wrong with the contact element update during restart.As I know I can stop the solution and restart from the last converged substep. I am trying to figure out why this is happening.Do you have any explanation about that? Do you thing your suggestion can solve that problem? I will try with that also.
Thanks
Mon

 

[Stringmaker]

Are you certain that you're performing the restart properly? I've never had the need to use the restart analysis type so I'm not that knowledgable. However, there is a checklist of things you should be certain to make sure are intact. The suggestions above were made with the thought of assisting you in getting better contact convergence. They may or may not help with your dilemma here. Trying is the only way to know. I'd speak with your Ansys support as there sounds like something isn't quite right regarding not being able to restart. I may be a bug of sorts but if the analysis solves to completion I wouldn't get hung up over not being able to restart. There's too much other stuff that needs done to worry about something which is somewhat trivial. As an aside, you may want to see the RESCONTROL command as the answer to your question may lay within. If you do figure it out please post the issue. I'm curious.

Good luck,
-Brian

 

[cbrn]

Hi,
I believe the key of the problem is in the first answer from Stringmaker: if your contact settings are such as to update the contact stiffness at each step, then what is happening is the following:
- in a single run (single step), the contact stiffness is evaluated at start, then the calculation proceeds to convergence following this value of stiffness.
- with a restart, the first part of the analysis is like above; at restart, instead, the contact stiffness will be re-evaluated and, depending on the stress / deformation state of the system, can give a value that is not compatible (or even incoherent), thus causing convergence issues or even mis-convergence.

The solution should be to ensure that the contact stiffness updates at each EQUILIBRIUM ITERATION (it will slow down the analysis, but it provides the most precise results).

Hope this helps...

Regards