Excessively Distorted Elements with General Contact in 2D Explicit?

[dfgsdfgfd]

I have a 2D lattice structure, where each strut consists of multiple beam elements (B22). The lattice is sandwiched between two plates, that compress the lattice. I run the simulation on Abaqus Explicit and apply General Contact. However, already in the very first computation, before the lattice is much deformed, I get excessively distorted elements (see pic below -- the beams are supposed to form a straight line between the nodes).

When I run the simulation with contact between the lattice and plates only, it works perfectly, but (obv) the beam elements are ghosting each other.
When I run the exact same simulation (with General Contact) in 3D, using B32 elements and BC to constrain the out of plane movement, it also works perfectly, but is much slower.

Is there a known bug or workaround for this? Thanks!

 

[FEA way]

Is the lattice modeled as a single part ? Did you try using tie constraints between the lattice and plates ?

 

[dfgsdfgfd]

The lattice is modeled as one single part (wire). No tie constraints, as the lattice needs to be able to slide on the plates as it compresses.

 

[FEA way]

Maybe the load is too high or too rapid. Make sure that all units are correct. Can you attach your model’s files (cae or inp) ?

 

[dfgsdfgfd]

Good points, the only thing is that it all works fine if I don't apply General Contact:

https://www.dropbox.com/s/rf5dzvy69fvc30b/model.cae?dl=0

Thanks for your help with this!

 

[dfgsdfgfd]

Does anyone else have an idea on how to solve this issue?

 

[FEA way]

Here's what you can try to fix this problem:
- check all warnings generated in output files, they may point to specific issues with the model
- make sure that beam elements have properly defined orientation
- use much coarser mesh and offset the plates from lattice (Abaqus assumes circular beam cross-section for contact and may automatically reduce contact thickness to prevent self-intersections)
- start from very simple model (like single lattice cell between plates) and see if it works properly

 

[dfgsdfgfd]

(1) the warnings showed lots of issues with overclosures

First, there's about 3000 messages like this:
Initial node-face overclosure is 1.4702 at node 537 of instance ASSEMLATTICE and face S1 of element 145 of instance ASSEMLATTICE

Second, there's another 3000 messages like this:
Adjacent slave nodes 9 and 10 of instance ASSEMBOTTOMPLATE may be on

Third, it then tries to fix the issue automatically. This might be the issue for the warping, but I don't know how to prevent it:
Initial contact adjustment is 0.62562 at node 20 of instance ASSEMLATTICE

Fourth, it then continues with:
Unresolved initial overclosure is 4.4367 between node 9 of instance ASSEMBOTTOMPLATE and face S1 of element 317 of instance ASSEMLATTICE

Fifth, it starts over again with #1.

I tried playing with all the different contact parameters and removed the plates, but neither of that resolved it. Also, I don't have the problem in the 3D simulation, so I assume it must be a bug.

(2) the beam elements' orientation is properly defined.

(3) having one beam element per beam/strut actually works! However, that's not really an acceptable solution for the accuracy I need.

(4) same problem as with the actual

I guess I'll just accept the fact that I cannot resolve the issue and will continue with the 3D model. Thanks again for your help.

 

[dfgsdfgfd]

In case other people are interested, the problem had to do with the cross-sectional shape of the beams, which had a high thickness-to-depth ratio in my case that messed things up.