Buckling analysis

[aharri]

Hi

I am doing comparison of buckling analysis of a plate structure. My structure (XZ) has constraint Y on sides and top, and pins on bottom. The load is set at top nodes as distributed load. When I do the same structure on RFEM5 and STAAD8 I get the same curve when I plot all the points, but the values are lower. Why is that?

Best regards
Antti Harri

Attachments:

You must be logged in to view attached files.

[NextFEM Admin]

Hello,
have you checked deformed shapes for local buckling modes?
If you’re interested in in-plane buckling modes, you should model the wall in XY plane and set elements as plane stress (Edit / Change element type).
To perform a proper comparison, please make sure the mode is treated the in same way.

[aharri]

Hello
Thank you for the quick reply.

When I visually examine the buckling shapes they match. Every program does things a bit differently, but I tried to model them all as closely as possible.

When I use the query tool, there is no type currently set for the triangles. After I rotated the model -90° around global X and changed the element types to plane stress I get the solver error below:

++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++
NextFEM Designer v.2.30
Model name: panel-3000x2000_grid-1000×1000-test
++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++
Number of nodes: 18
Number of elements: 24
Problem size: 144
Number of restraints: 12
++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++

++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++
Starting analysis for case Wind +X
++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++
Collecting model data… Done.
Launching…
Solving …
Real time consumed: 000h:00m:00s
User time consumed: 000h:00m:00s

++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++
End of execution for load case Wind +X
++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++

++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++
Starting analysis for case Buckling
++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++
Collecting model data… Done.
Launching…
Assembling stiffness matrix
Assembling variable loading
Solving linear static problem
Assembling initial stress matrix for variable loading

Error:Method computeInitialStressMatrix is not implemented

++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++
Execution finished at 01/16/2024 19:55:20
++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++

[NextFEM Admin]

Hello,
can you please share the model to let us have a look?

Why not using quad elements?

[aharri]

Hi

Yeah sure, I attached one of the models.

The quad elements gave very low buckling factors such as 0.200.

Best regards

Attachments:

You must be logged in to view attached files.

[NextFEM Admin]

Hello,
we fixed a bug on quad elements that was causing the low factor you got – we’ll release the fix during this week, hopefully.
Regarding the comparison, results depend also on mesh fineness. We suppose you have the same mesh size and load (20kN) on all models. Another thing that affect results is the element formulation: in the built-in solver, tria elements are built by a membrane and plate, while quad elements have MITC4 formulation, which is generally more reliable.
Before releasing the patch we’ll do a parametric test on shell buckling, we’ll let you know when the update will be available.

[aharri]

Hello

Thank you and I’m glad that my feedback resulted in finding a bug.

Yes, I have the same mesh size and loading, although in RFEM the supports have the type of “line support”, which propably translate to mesh nodes having node support.

Would I be able to use just one quad element and have fine mesh for calculation? When I was trying it with this method, it calculated strentgh from the element and mesh -> intersection capacity was doubled. Then I ended up doing one quad element, dividing it, meshing it so that triangles were used and I deleted the original quads. This way I could have visually pleasing mesh created.

Best regards

[NextFEM Admin]

Hello,
please try version 2.3.0.3; the patch for quad elements has been released. For tria, we’re still getting lower results, we’ll get in deep. For quads, we get a good agreement with results you already have. Always use a proper mesh (at least 5 quads per side).

You can also run a parametric analysis automatically with Python in this version, please see the sample at https://github.com/NextFEM/API-Python/blob/main/wall_buckling.py

[aharri]

Hi
I tried it and verified it now gives the same result on quad at least for one case. But there seems to be some occasional errors when solving the model, and I can’t pin-point why. Sometimes re-running the solver works. Another example: I took one model that had 1000×1000 elements and I kept dividing them, and at smaller size the solver refused to work (I think it was 50×50 or 100×100).

Unfortunately my license doesn’t allow parametric solving and I do not have python extension installed.

What about 3d solids? With them I get very high buckling factors. Maybe verify those work too, after the quad and tris are sorted.

PS. Could the download-page say which sub version it is, too?

Best regards

[NextFEM Admin]

Hello,
please upload your non-working models with shells and a sample with solids at the bottom of the Support page.

No, the complete versioning cannot be written in the download page, that page always hosts the latest version. You don’t need to use it to upgrade, simply press Updates / Check for minor updates… in the program!

[aharri]

Hi

I will upload them a bit later. If you are interested, here are the results of my analysis with plates/surfaces in various programs. Nextfem is now very consistent with RFEM, when using quads (50×50). Only interesting thing I noticed based on the analysis, is that Staad calculates buckling differently with very narrow models, please see “1000.png” that is attached.

Best regards

Attachments:

You must be logged in to view attached files.

[NextFEM Admin]

Thanks for your comparisons. We corrected buckling on tria, this will be released in the next patch.
As we use OOFEM as default solver, we forwarded your check request to OOFEM team.

ps. please upload one model with solid elements just to see your assumption about restraints and loading; other solvers confirm the correctness of OOFEM approach to solid buckling.

[aharri]

Hi

Model attached. The restraints differ a bit in comparison to the surface models, as the solid model has some eccentricity. Should this be modeled with two layers of solids and then the supports will be in the middle nodes? Although I don’t believe this is the reason for such high difference in buckling factors.

Best regards

Attachments:

You must be logged in to view attached files.

[NextFEM Admin]

Hi,
thanks for sharing the model – indeed the eccentricity plays an important role, please note that in the static loadcase you have out-of-plane displacements.
As told, we get the same buckling factors with other solvers (we used CalculiX) – you have to consider that you’re using distorted hexa elements: 1 dimension (thickness) is much shorter that the other 2, hence the elements is not in its ideal condition to work properly.

[aharri]

Hi
Yes but if anything the eccentricity should decrease the buckling factor, not multiply it by a factor of 10. Also, it is very little (4 mm) off center.

For the next stage of my thesis work the solid model could be more useful. Could you please suggest how it should be modeled in NextFEM? Will it be enough to just make the element proportions closer together?

Best regards

[Author]

Posts