Contact Problem - Deformable to RS
Contact Problem - Deformable to RS
(OP)
Dear forum members.
I would really appreciate any suggestions on overcoming a contact problem. I'm modelling the installation of a seal between a shaft and a cover. Shaft and cover are modelled as rigids and installation is done in 2 steps (step-1: install shaft, step-2: install cover.
My problem is, when the shaft starts to move to the installed position, it pushes the seal towards the cover. The outermost node of the seal seems to be having a contact ctrl with the cover (RS) and the job shuts down. The node has a stress value eventhough it hasn't even come into contact with the RS!
I have checked the surface normal of the cover, looks like the right one. Also created contact ctrl for the interaction, but that doesn't seem to work.
Can anybody please give me any suggestion, or explain more about contact ctrl? I usually use friction=delayed, and auto stabilization. I'm a relatively new Abaqus user.
Thanks a lot in advance.
jo
I would really appreciate any suggestions on overcoming a contact problem. I'm modelling the installation of a seal between a shaft and a cover. Shaft and cover are modelled as rigids and installation is done in 2 steps (step-1: install shaft, step-2: install cover.
My problem is, when the shaft starts to move to the installed position, it pushes the seal towards the cover. The outermost node of the seal seems to be having a contact ctrl with the cover (RS) and the job shuts down. The node has a stress value eventhough it hasn't even come into contact with the RS!
I have checked the surface normal of the cover, looks like the right one. Also created contact ctrl for the interaction, but that doesn't seem to work.
Can anybody please give me any suggestion, or explain more about contact ctrl? I usually use friction=delayed, and auto stabilization. I'm a relatively new Abaqus user.
Thanks a lot in advance.
jo





RE: Contact Problem - Deformable to RS
Can you run the analysis without using the contact controls? Most of the time, ABAQUS does a reasonable job without having to tweak them in my experience.
If the analysis fails to complete, what is the error message that you get? What sort of analysis is it - 2D, 2D axisymmetric, 3D? Explicit or Standard?
Regards
Martin
RE: Contact Problem - Deformable to RS
It's a 2d axisymmetric, std analysis. Seal is rubber, Marlow model. I have 3 models to analyze: nominal, max and min. Default settings seemed to work well with nominal geometry, but do not work with max and min.
Contact ctrls did the trick for the max geom, which is why I'm tweaking the same thing for the last one (min).
The error msgs I get are
- THE SYSTEM MATRIX HAS 1 NEGATIVE EIGENVALUES.
- SOLVER PROBLEM. NUMERICAL SINGULARITY WHEN PROCESSING NODE
What does it mean by numerical singularity?
Thanks a lot,
jo
RE: Contact Problem - Deformable to RS
Might be that the outermost node is getting 'stuck' for some reason. Maybe try running the model with zero friction and see what happens?
You say that the shaft & cover are modelled as rigids - are they analytical rigid or meshed rigid (RAX elements)?
Regards
Martin
RE: Contact Problem - Deformable to RS
The shaft and cover are analytical rigids. I wonder what causes the problem... the offending node does not even belong to the seal. It belongs to a washer that is installed in the same cavity, sort of a backup seal. And the washer doesn't even get deformed.
thanks a lot,
jo
RE: Contact Problem - Deformable to RS
But I really appreciate the suggestion. Thanks, Martin.
regards,
jo
RE: Contact Problem - Deformable to RS
Might be there's a rigid body motion there somewhere if the washer is not fully constrained?
Regards
Martin
RE: Contact Problem - Deformable to RS
thanks,
jo
RE: Contact Problem - Deformable to RS
Can you run the analysis without the washer?
Regards
Martin
RE: Contact Problem - Deformable to RS
I tried lessening the friction coefficient from 0.05 to 0.001 and relaxing the slip tolerance (0.005 to 0.5). This pushes the analysis a bit further (0.7 step time).
Looks like the seal has a problem sliding on the rigids. Contact is made at 3 areas on the seal.
I hope someone can give me new suggestions. Thanks in advance.
regards,
jo
RE: Contact Problem - Deformable to RS
Is the washer modelled as analytical rigid aswell? Just a thought, but you cannot have contact between analytical rigids in ABAQUS, not with contact pairs anyway..
You could try posting the input file on a file hosting site like www.yousendit.com - I could have a quick look at it.
Regards
Martin
RE: Contact Problem - Deformable to RS
Finally cracked this one this evening!
Lessened the friction and loosened the slip tol, plus added a contact ctrl in the problematic step. That finally did it!
To answer your q, the washer is modeled as a deformable, but the material is a bit more rigid than the seal. I cannot post the input file publicly because it's proprietary info, I'm sorry.
I can give you the assembly and steps input, though, just not the geom bit.
But thanks a lot for your suggestion. Tweaking the friction was a really good idea. I shall forever be indebted to you :)
eternally grateful,
jo