distortion in Aabaqus

[Hamza 13]

Hello,
I have some problems with my Abaqus model, the job ran successfully and complete the time but the result is not as desired, the model shows a deformable shape and the hysteresis curve failed to get symmetrical loops.
the model is a metallic damper under cyclic loading.
step= static general, load: fixed end at left, loading at right (cyclic loading as tabular data) contains three different amplitudes, each amplitude was repeated 3 times, and sliding hinge either in the right(all fixed except the loading direction).
mesh: C3D6 is used ( sweep wedge elements) were no errors or warnings by using the mesh verify tool.
looking for your answers, and suggestions to get the right result.
pic attached shows the deformable shape of the system as shown there was buckling in the steel core and that is the cause of not getting the right hysteresis curve.
Best regards.

 

[FEA way]

Some details are necessary to provide help. Please describe as many features of the analysis as you can and possibly attach some screenshots (showing the model, mesh and those distorted results). For example, what is the step type, boundary conditions, loads, element type, material model, interactions and so on ?

 

[Hamza 13]

i edited the post
Chaboche model was used for the cyclic hardening of the steel core.

 

[FEA way]

Is that deformed shape shown in true scale ? With properly defined interactions there shouldn’t be such penetration. I assume that there’s a cutout for the core in the casing. It’s likely that the large difference in mesh densities of both parts causes failure of contact detection.

 

[Hamza 13]

Yeah I think it's problem of meshing ,but it's hard to mesh the core part because of the re_entrant honeycomb holes and especially those sharp angles ,the core part need a pro mesh can't find the appropriate one I try with hex but failed even with partitions, whats your suggestion for meshing this system ?

 

[FEA way]

I would rather focus on the mesh of the casing for now. It's very coarse and this difference may cause the problem with contact. Try significantly refining the mesh of the casing, leaving the core as it is.

P.S. It's an auxetic damper, right ? At first, I haven't noticed that the core uses re-entrant unit cells.

 

[Hamza 13]

Yes its core with auxetic structure, I try with another mesh, this time all the parts using wedge elements with 15 mm but the problem doesn't change ,every time with this penetration don't know why ?! As shown in the curve ,model start buckle after few cyclic loadings.

 

[FEA way]

Try with general contact instead of contact pairs but also make sure that the initial state of the model allows for proper detection of the contact - for example, there are no significant overclosures.

 

[Hamza 13]

it's was a problem of contact, but I didn't create general contact, I just checked the box of the adjustment and prevented overclosures between slave and master surfaces in the interaction between the core and the restaining, so after that, I didn't get any penetration anymore.
but I have a question about the mesh, Are the wedge (sweep)elements bad for the accuracy of the results? because for a steel core full of re-entrant honeycomb holes, the hex meshing was so difficult, and even if I try it the running reaches a certain point and then failed, is it normal for this difference between the mesh results?