Partitions with same section results in stress discontinuities at the interface

[xarz]

As the title explains, in my abaqus model I've a part that is split in two regions by a partition. For each region I've defined the same section separately (i.e. I've assigned an "A" section to the first region, and then the same "A" section to the other region). The analysis shows a gap in the stress (mises) field and I really can't explain why. The section (so the material) is the same, the regions have the same finite element mesh, so no discontinuities can be justified. Is this a solver issue or it's my fault in modelling the element? Is there any workaround?
If assign the section at the same time to both the regions abaqus shows no discontinuities.

Thanks.

 

[IceBreakerSours]

Interesting. I do not know the answer to your question but I am curious to know a few things:

If you the same material defined and no change in mesh in those two regions, then why did you create a partition in the first place?

Do you care about the stress discontinuity near the partition? Isn't it far enough from the location of contact?

If you do care about it, how significant is the discontinuity compared to average values in the neighborhood of the discontinuity?

Finally, have you made sure there is no change in element formulations in the two regions?

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

 

[xarz]

Hi, I have created this partition because the most superficial layer must be of a different material. However since I was experiencing stress discontinuities I thought to test abaqus behaviour using the same material in order to exclude possible errors in the model definition. However I was expecting to obtain no discontinuities but these are still there. The two parts are meshed in the same way as can be seen in the image. This problem makes me worry about possible errors in abaqus computations when using regions separated by a partition. In the specific analysis I'm looking for how rebounce speed changes changing the thickness of the superficial layer, so the behaviour at the interface can definitely influence the analysis result if thickness is small enough.

 

[IceBreakerSours]

a) Check your INP and ensure you have the same element type in the two regions.
b) If they are, try refining the mesh.

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

 

[xarz]

I've checked and I'm sure that the two regions have the same element type. Also refining the mesh hasn't helped. I do not know what to think anymore..

 

[IceBreakerSours]

Have you tried getting rid of the partition? Also, if you like, you can upload your CAE.

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

 

[xarz]

thank you very much for your kindness, here is a zip file with the .cae inside.

Download Link .cae

If you try to run the analysis you will see some warnings that can be ignored (like a null density warning: I've defined the mass of the impacting mass using the engineering features and so I've set 0 density in the material properties),

ps. If I remove the partition there is no more a gap in the stress field. But I need that partition.

 

[IceBreakerSours]

You do not need a partition simply to define a different material property to a few elements.

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

 

[xarz]

So how can I do that?

 

[IceBreakerSours]

Please go through a couple of step-by-step examples in the documentation.

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

 

[MechIrl]

BTW (from you CAE file) your use of elements is very inefficient. There is no reason for using 1.e6 elements in a problem like this. Look at using mesh refinement and symmetry to reduce your problem size (which would also allow more elements in the contact area than you have). You can assign different sections to individual elements in orphan meshes if you don't want to partition.

 

[IceBreakerSours]

I believe I have found the reason for the "discontinuity". Since you chose two different sections, Abaqus "thinks" the nodes at the interface belong to two different result regions, and therefore, applies different averaging coefficients - which makes it look like a stress discontinuity.

Abaqus CAE User's Manual section 42.5.2 (for v6.11):

"Abaqus/CAE averages values at nodes common to two or more elements when the contributing elements lie in the same result region. The default result regions are the same regions defined when you assign sections to your model; you can also define custom result regions using saved element sets or display groups. You can choose whether or not Abaqus/CAE averages values at nodes common to two or more result regions. You can suppress averaging across regions (use the region boundaries) to emphasize any discontinuities at region boundaries, or you can request averaging across regions (ignore region boundaries) to produce a more continuous effect."

~!ce.

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

 

[xarz]

I'm really aware that the meshing I've used in that .cae is very inefficient, but that mesh was only one of the ways I used to understand what was creating the discontinuity in stress field as I've reported before. I tried to use such kind of meshes to exclude the influence of meshing itself in this problem.

The fact is that I can't explain why a partitioning automatically produces a discontinuity in stress field. It should not happen if I assign to both regions the same section-material.

If you've seen my .cae file, have you any idea of what can give such a behaviour?

 

[xarz]

@icebreaker
I'm analysing what you've suggested. I'll report back here once I've investigated. Thanks a lot for your efforts.

 

[xarz]

@icebreakersours

Thanks a lot. That was the reason.

Turning off "use region boundaries", under "computation" tab in "result options" window, has done the trick.

Really thanks for sharing your knowledge and time.

I wish you a good day.