Intersecting instances in contact analysis

[Staszkinson]

Hello
My question is about contact problem using C3D8R elements, surface to surface contact, hard contact.
I have made simple t-stub model. Included images show effect of the analysis in two ways - with different scale factors(1:1 and 5:1).

What do u think about second image, is it ok that in high scale factor two elements/instances intersect each other?

Thank You.

 

[IceBreakerSours]

is it ok that in high scale factor two elements/instances intersect each other?

Intersection of elements makes no physical sense. Scale factor is simply for visualization. If you are not sure about this, you must review the theory of FEA!

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[Staszkinson]

Thanks for the answer.
Have You ever got the same problem in contact analysis?

In the other analysis, I put the instances at the same points and adjusted to remove overclosure, then i put the bolt load. The results are in the included file(very high scale factor). As You can see there is no overlapping. That is what I expected and I suppose it's correct.

Unfortunately if I supress bolt load, there is a problem with overlapping(post 1).

Have you any ideas?

 

[corus]

The difference between the pictures, and presumably the models, is that you have two different meshes. In the latter the mesh of the two 'slabs' is of the same density, whereas in your original post, the meshes differ. One may appear to intersect another as the slave nodes can pass through the master surface (or is it the other way round?). As such one mesh appears to pass through another at a high scale factor. It would be better to have similar meshes between the two parts to get better contact interaction, or define another contact pair of the same surfaces but with the master and slave surfaces interchanged.

 

[Staszkinson]

Thank you for the answer.

As far I know(I have read manuals), I found that it is recommended to mesh the slave part with more detensity.

or define another contact pair of the same surfaces but with the master and slave surfaces interchanged.
Unofrtunately didn't help.

I suppose that this problem is about influence of seperation two instances at the beginning of the anaylysis.
Included image should help you recognize what I'm talking about:
1a and 1b - the same mesh detensity, overclosure removed at the beginning of analysis(OK)
2a and 2b - different mesh detensity, overclosure removed at the beginning of analysis(OK)
3a and 3b - different mesh detensity, overclosure IS NOT removed at the beginning of the analysis(PROBLEM)

 

[corus]

In the latter case you clearly have an initial gap before contact is made. When you scale up the displaced shape by a large factor then the displaced shape will appear to pass through one another.

 

[IceBreakerSours]

The following is from the ABAQUS Analysis User's Manual:

1. The larger of the two surfaces should act as the master surface.
2. If the surfaces are of comparable size, the surface on the stiffer body should act as the master surface.
3. If the surfaces are of comparable size and stiffness, the surface with the coarser mesh should act as the master surface.

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[Staszkinson]

Thank all of you.
Icebreaker: my project pass requrements from 3), on my images, bottom instance has master surface
Corus: i stiil think that it isnt ok. Even at scale 1:1 I can observe intersection. Thank you.

I need to verify my model.

 

[3JC]

Dear Lukasinski:

It could be possible that a refined mesh give you better results. Also you can try with the stabilyzation of the step (damping factor, for example).

 

[Staszkinson]

Thank You for the answers,
I have checked my model and now, I'm sure that Corus was right. At big scale factor is ok that two instances are interesecting each other.

Thank You.

 

[Staszkinson]

And one more question.

How should I interpret a grey colour in the visualisation module?
It isn't at legend box.

It's is overall question. Sometimes in the stresss analysis, in the visualisation module I get grey colour too.

Thanks.

 

[Staszkinson]

File in the attachment.

 

[corus]

Grey is the colour above the maximum value you've chosen in the legend.