Contact convergence 2

[krishna1]

Dear All,

While doing the contact analysis(Using Ansys), the common problems i am facing are with the convergence of the model.

i) I regularly use point to point contact elements and try to converge the problem(Number of elemnts in my model usually be around 200000), but most of the time i am failing to converge the model. Then i use weak springs with very low stiffness. What i couldn't understood is that a finite number of weak springs with a very low stiffness of "1" will converge the model.Can any one suggest me on this and some tips for getting the model converged.

ii) Will the mesh pattern aroung the contact region will cause a great concern in convergence ?

Thanks and Regards,
Krishna

 

[nikolas]

Krishna, this is what i have intrepreted from your first part of the question, please go through it and correct me if i have intrepreted it wrongly.
Well krishna the first part of your question tells me that using low stiffness spring elements converges the model and gives you the answer but friend the answer in this case would be wrong. Because there is a direct proportion between the stiffness and the convergence rate of the solution because its obvious that as you increase the stiffness the model will take time to converge. Secondly, by using low stiffness you are allowing more penetration which means that the answers would be absurd.

 

[krishna1]

Nikolas,

Thanks for the response. Let me write the question clearly. I am using the weak springs along with the contacts. I am not getting the convergence with contacts alone, where as the convergence is done with contact elemnts along with springs of low stiffness.

I hope you understnad the problem. Please throw some light on to this.

 

[nikolas]

I would recommend you in this case to start with low stiffness contact elements and then go on increasing the stiffness of the contact elements. compare the answers you get each time. It might be that Ansys would be solving the problem with high stiffnesses assigned to the elements either supplied by you or calculated by itself and so the problem is not converging.
If the high stiffness of contact elements is a problem then solving the problem with low stiffness contact elements should converge the problem and give you the answer (Well but in this case the answer may not be correct!!!!)

 

[convergence]

prove whether the magnitude of the primary variable solution based upon the finite element method will converge to the exact solution from above or below

 

[tld23]

krishna1,
The reasion for non-convergance of contact are many. However many are solved or at least helped by trying a few simple things:
1) Make sure your master slave surface is the correct way around, make sure the larger elements are on the master surface or that any rigid surface is the master.
2) Make sure that the slave surface does not "hang-off" the edge of the master.
3) Use displacement loading whenever possible, even if it is to pre-load the contact befor swapping to force load.
4) Over-load the joint using a displacement load, then swap to a force load that is too high and finally reduce the force to the required load. This is only applicable if the materials are elastic and friction is low.

Hope these suggestions help.

TERRY

 

[corus]

I would add to tld23's comments by saying that better convergence is obtained by using linear rather than quadratic elements. Additionally it is better if you have the same mesh density for both surfaces otherwise select the master surface based upon the coarser mesh. Equally if one surface material is softer than the other then make this the slave. You can also modify the convergence criteria to stop "chattering" of surfaces.