Contact Problem - Deformable to RS

[mizzjoey]

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

 

[bassmanjax]

Hi Jo

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

 

[mizzjoey]

Thanks Martin for your reply.

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

 

[bassmanjax]

Numerical singularities - Cansand summed it up nicely in a previous post;

Numerical singularity would mean zero stiffness which in turn could be due to insufficient constraining of the material, buckling of a point in your system (geometry -caused such as a weakness pont (imperfection) or it could be due to the high distortion of the material point.

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

 

[mizzjoey]

Good idea, I will try with zero friction this time.

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

 

[mizzjoey]

No luck with the zero friction approach
But I really appreciate the suggestion. Thanks, Martin.

regards,
jo

 

[bassmanjax]

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.

Might be there's a rigid body motion there somewhere if the washer is not fully constrained?

Regards

Martin

 

[mizzjoey]

Hmm... I have created a hold BC for the washer and the BC is removed in the second step. Are you saying that I should maintain the BC til the end of the job? I could try that. The analysis does have a problem in the step where the hold BC is removed.

thanks,
jo

 

[bassmanjax]

If the washer is unconstrained, either using a boundary condition or contact condition with it's surroundings, then it will just 'float' off and potentially throw a singularity error.

Can you run the analysis without the washer?

Regards

Martin

 

[mizzjoey]

Nope. Washer has to be included because the seal is supposed to deflect, which is also due to the presence of the washer.

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

 

[bassmanjax]

Hi Jo

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

http://www.yousendit.com

- I could have a quick look at it.

Regards

Martin

 

[mizzjoey]

Hi Martin.

Finally cracked this one this evening! :-D
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