Help with understanding non-convergence?

Wesley Peijnenburg

I'm using tutorial OS-T 1394 and 1560 (V2022.1) and made a similar model from scratch to check if I understand it. Hopefully someone is willing to help with understanding a non-convergence problem?

Attached is the model, the purpose is to simulate contact between a sphere and wall (axisymmetric). 

There is a very good blog post which helped me a lot: 
https://community.altair.com/community?id=community_blog&sys_id=538764ab1b3790d4a5f742eddc4bcba4 

Thanks to the blog post I could already try the below corrections to solve it:
   - Following advice found in output file, friction has been set to zero.
   - Contact stabilisation: CNTSTB with parameters from OS-T 1560. Goal is to find stress fields, impact on energy accuracy can be accepted?
   - Tried increasing force
   - LS input DLOAD - This seems to solve warning 1955 "zero static force vector"?
   - It gives info 4936: suggested TLOAD1/TLOAD2. Indeed works fine but does not solve the issue.
   - It does seem to solve error 1996: "All entries have zero scale"
   - Error 941 now remains: non-convergent iterations

Possible reasons that I can think of:
   - Force 0.2N not properly applied?  
   - Not properly constrained?
   - Insufficient/poor elements for the wall part?
   - LGDISP needed to capture deformation? 
   - Convergence expert keeps backing off, but why? Step too large? 

Important warnings that remained: 
WARNING # 3400 - Singularity detected at following 1 DOFs.
WARNING # 6529 - The x-displacements of grids (e.g., GRID 1) on the axis of symmetry need to be constrained  ->

Many thanks in advance! 
- Wesley

Robinson Ferrari_20451

Hello Wesley,

I needed to do some changes to get your model converged. So, please check both models and try to understand the differences. You can use this article from our community as a reference for the debugging model. https://community.altair.com/community?id=kb_article&sys_id=a6b1eafedbfd4d10cfd5f6a4e2961906
Also, I would like to recommend that you enroll in one of our OptiStruct non-linear online training sessions.

1) Fix your material data, be sure you are using consistent units (I have scaled your model by 1000x and I used MPa)

2) Swap Main and secondary surfaces (the finer mesh should be secondary surface)

3) Use discrete CONSLI (continuous sliding) in the LGDISP approach. For this model, it can be small sliding works for you however, be sure the slide distance will be less than 1 element size and you are using the right search distance

4) Prefer using penalty = SOFT in PCONT (if you see any huge penetration you can change it to AUTO)

If it works for you, please mark the answer as correct for helping others.

Thank you very much,

 

 

 

Robinson Ferrari_20451

Hello Wesley,

I needed to do some changes to get your model converged. So, please check both models and try to understand the differences. You can use this article from our community as a reference for the debugging model. https://community.altair.com/community?id=kb_article&sys_id=a6b1eafedbfd4d10cfd5f6a4e2961906
Also, I would like to recommend that you enroll in one of our OptiStruct non-linear online training sessions.

1) Fix your material data, be sure you are using consistent units (I have scaled your model by 1000x and I used MPa)

2) Swap Main and secondary surfaces (the finer mesh should be secondary surface)

3) Use discrete CONSLI (continuous sliding) in the LGDISP approach. For this model, it can be small sliding works for you however, be sure the slide distance will be less than 1 element size and you are using the right search distance

4) Prefer using penalty = SOFT in PCONT (if you see any huge penetration you can change it to AUTO)

If it works for you, please mark the answer as correct for helping others.

Thank you very much,

 

 

 

Wesley Peijnenburg

Robinson Ferrari_20451 said:

Hello Wesley,

I needed to do some changes to get your model converged. So, please check both models and try to understand the differences. You can use this article from our community as a reference for the debugging model. https://community.altair.com/community?id=kb_article&sys_id=a6b1eafedbfd4d10cfd5f6a4e2961906
Also, I would like to recommend that you enroll in one of our OptiStruct non-linear online training sessions.

1) Fix your material data, be sure you are using consistent units (I have scaled your model by 1000x and I used MPa)

2) Swap Main and secondary surfaces (the finer mesh should be secondary surface)

3) Use discrete CONSLI (continuous sliding) in the LGDISP approach. For this model, it can be small sliding works for you however, be sure the slide distance will be less than 1 element size and you are using the right search distance

4) Prefer using penalty = SOFT in PCONT (if you see any huge penetration you can change it to AUTO)

If it works for you, please mark the answer as correct for helping others.

Thank you very much,

 

 

 

Thanks so much, especially because clearly effort was needed for the corrections. Marked as correct.

You are right, completing relevant courses first is indeed a better approach. I'll enroll into the online training before posting more.

Still struggling a bit to understand the remaining differences in attached (current) model:
1. Nodes were renumbered. Was this for convenience or does it impact computability?
2. Mesh moved away from Y-axis (smallest x coord = 0.1), why? Did you also move the axis of symmetry to 0.1 to keep the sphere solid (couldn't find it)? 
3. Additional constraints are added (I see 115 instead of 66). But they look like duplicates of the original constraint which fixes all nodes of sphere center in radial direction? Seems I'm wrong here. 

I could not find above differences due to lack of experience and probably missed some differences. Definitely need to enroll into the training, sorry to have asked unnecessary time from you and coleagues. 

Robinson Ferrari_20451

Hello Wesley,

You can post and ask more, no worries. It's a pleasure to help you.

Enrolling in the training will be good for you because everything will be covered there and you will have access to all the training material as well. There is a lot of good information there.

1. You don't need to renumber the model, I have done this only for checking.

2. After scaling 1000x the model, I moved it only for having all nodes in x-y positive plane, otherwise will get an error message.

3. It should have only 51 SPC DOF1 (even if duplicated only DOF1 the results will be similar).

4- Finally, in the original model you were applying a force at a node out of the sphere, so nothing was happening (no forces applied).

Thank you