Convergence for Contact

[ajroman]

I am having trouble with getting my model to converge during a static, general contact problem. Does anyone have any tips/suggestions? I have tried to reduce the initial and min. increment values but I have gone as far as I can compute (e-40) and received an error message stating the increment value is too small.

Also, I have established a standard general contact interaction in my initial step, do I need to add additional contact interactions in the following steps? Wouldn't this just add to the complexity of the problem and further add to the computation?

Any help is much appreciated. Thanks.

Additional information related to this problem can be found in the following threads:

http://www.eng-tips.com/viewthread.cfm?qid=255686&page=1

http://www.eng-tips.com/viewthread.cfm?qid=255917&page=1

 

[rstupplebeen]

Can you post your model?

Try turning automatic stabilization on in the step but make sure to check your energies for error associated with it. Excessively small step sizes usually don't help. I find a minimum increment size of 1e-8 usually works for what I do. If it doesn't going smaller does not help usually.

I hope this helps.

Rob Stupplebeen

 

[ajroman]

I can't upload the file to engineering.com. I believe the file size is too large to upload (14 MB).

I've tried using automatic stabilization for both the initial and first step of the analysis and still no luck with convergence. Is there another way I could pass along this file onto you to take a look? Thanks again for all your help with this problem.

-Anthony

 

[rstupplebeen]

Try deleting anything you don't need and then do a save as. CAE keeps a bunch of baggage in the file that gets wiped out with a save as. If that doesn't work delete the meshes and do another save as. If those don't work send the INP file.

Rob Stupplebeen

 

[ajroman]

Please use attachment below to view file. Thanks.

 

[rstupplebeen]

Here is a running list of my thoughts on your model:
1. Wow that's a lot of plies (21) to try on the first attempt!!
2. The mesh is very coarse on each fiber
3. Your top and bottom plates can be 1 rigid planar element each
4. Is the uncured carbon really that stiff?
5. Since you only have 1 interaction property and you have general standard contact you don't need the additional ones for contacting the plates
6. Your load is being overridden by the displacement constraint
7. I am not sure what BC-2 does
8. Every cut face of the fibers should have a constraint in the normal direction.
9. There are no rotational DOFs in a solid model so you do not need to constrain them (Abaqus ignores them)
10. You will probably need rigid vertical walls for the characteristic element to contact.

I hope this helps

Rob Stupplebeen

 

[ajroman]

Response on thoughts:

1. I agree, should I breakdown the analysis into additional steps to improve results/help convergence?
3. Would reducing the plates to planer elements help in the analysis step by eliminating additional computations?
4. Surprisingly yes.
7. This boundary condition was supposed to restrict the model's movement in all directions except in the 2 direction (just allowing compression of entire model).
10. In one version of the analysis, I had walls. But due to convergence concerns I removed them and added BC-2. Could these walls also be modeled as a rigid planar element?

 

[rstupplebeen]

1. I meant to try only a couples of plies during this error checking phase then add in all the plies for the final analysis.
3. Very slightly. I basically just think it looks cleaner.
4. I have worked with a lot of dry carbon and prepreg and most were limp (frozen prepreg has some stiffness to it). You might be applying tensile data which will give spurious results for bending.
10. Rigid planar elements should work. There is an assumption that this plane will represent symmetry not cyclic symmetry.

Rob Stupplebeen

 

[LTB]

Good afternoon,

I liked that I could solve a problem that I have in Abaqus. The model I'm preparing can be downloaded at this link:

http://ftp.ua.pt/incoming/fghj/.

As you can see through the file is a model consisting of eight cells of cork that are restricted and are under the action of a shift that originates compression. My problem is related to the fact that the top faces of the cells intersecting the lower cells, which can not happen. Can anyone help?

Thank you for your attention

Greetings