This content has been marked as final. Show 5 replies
I am not a place where I can look at the clip analysis right now. I will look tomorrow.
1. Are you using friction at the contact areas? I noticed the same problem without friction is 10 to 20 fold faster.
2. Did you set a small max time step?
3. Did you tighten the convergence tolerance?
4. Do you have "Stiffness singularities, Non-converging gap" errors?
5. What solver are you using? Try the iterative solver to for speed improvement.
I am betting you are having similar problems with the "No penetration" contact that I am. It seems to get to a certain point and just stop the analysis. It keeps cranking away but eventually gives the error "Stiffness singularities, Non-converging gap." I was able to remove contact as a more crude approximation in my model which allowed me to use "Arc Length" control instead of force. This allowed me to get a solution.
Download procexp.exe from www.sysinternals.com . Run it while cosmos is running the nonlinear analysis. Double click "Nstar.exe" and see what kind of processor usage you are getting. Process Explorer is way better than window's task manager.
More to come later. I just need more info.
1. No, I am not using friction at the contact areas
2. I set the max time step at 10% of my final time
3. I left the convergence tolerance at the default
4. I do get stiffness singularities and Non-converging gap errors
5. I'm using the direct sparse solver
One thing I think I may have done wrong was enter the strain values for the stress strain curve as numerical values instead of percentages. ie. I entered .1 instead of 10. Can some confirm what numbers it is looking for when entering stress-strain data?
I've been using a non-linear elastic model for Delrin 500, but I'm not sure that is the best option. Does anyone have any thoughts on the best material model to use?
without knowing much else about your problem I would say that a good choice for Delrin would be the NL Eleastic model - assuming you are not all that interested in the "recovery phase".
You need to enter the stress strain curves as stress whatever unit you are using psi MPa whatever and strain is in real numbers - like 1% strain would be entered as 0.01. The other thing is that you should use true stress strain curves. True stress strain curve can be easily calculated from engineering stress strain curves - just google it to get the relationship.
Non-linear with contact in Cosmos, while it can be made to work it is very very often a try this and try that and pull your hair out sort of endeavor. Frankly, it isn't Cosmos's best game by a long shot. The "static" solver is much more robust in handling contact but that doesn't really help much when you need the NL capabilities. For that matter contact is pretty hard with any code and being restricted to tets doesn't help the stability issue.
What you might want to do is run a linear material model and see if you can tune the contact to work well and fast and try the NL material model.
Your mesh is not good enough. Check the mesh plot type jacobian. This gives you an idea of how distorted the elements start out. CosmosWorks does not remesh after each step to avoid distorted elements. Distorted elements cause stiffness singularities as well as errors in the results. For more info, check this topic: