Large Global Fea model buckling analysis

[cyt4]

Hi, I have been an avid fan of this forum for quite a while. I am currently analyzing and sizing a wing leading edge structure in femap and nx nastran. The structural static analysis is running fine whereas extracting buckling loads is proving to be an issue. Nastran almost requires >150gb scratch file which is breaking down the buckling analysis. Is there any way to break down the global fea vehicle model into smaller chunks to find the eigenvalues without sacrificing the accuracy? I am only interested in getting the buckling modes of the leading edge. Thanks in advance.

 

[rb1957]

you can divide up your model with NASTRAN superelements, but I'm not sure if this is compatible with buckling analysis. It sort of makes sense that things you have modelled as superelements won't buckle (only the detail model would be analyzed) so if there's a specific area you're concerned about you could focus on that and use superelements for the parts of the structure you're not concerned about. but it may be a simple "no go" ... no buckling analysis allowed with superelements.

but I wonder if you can trick it and replace the superelement with a very simple model that has the same stiffness as the superelement ?

another day in paradise, or is paradise one day closer ?

 

[cyt4]

interesting idea. well i have tried couple of options: analysis sets and freebody cutout. Analysis set got quite large quite quickly in the order of >150gb.The cutout seems to be the more sensible approach as it preserves the element loads, boundary conditions and applied loads.However, if you are not careful in selecting edges(edges being close) there are artificial buckling modes at the boundary. Most of the modes were junk. I will give the superelement a go but i might need to read up on superelements as I havent used them in the past. Thanks for the idea.

 

[namklof]

You might also try a difference Eigensolver. Inverse Power Method (SINV) is supposed to be for efficient for large models than Lanczos.

 

[cyt4]

So we have solved the problem. The best way to tackle the problem is using the aset in nastran. It is quite powerful and lets you have your results quite quickly. The run times dropped from 1.5 hours to 3 mins per case. The values actually correlated well with the global buckling runs. Setting up the model for breakout might take sometime but it is worth it if you have more than 10^6 degrees of freedom.

You have to set up your model with couple of constraints and loads. I did this in FEmap so this is how it goes.

- Make a group of your interested region(aset) and another one(breakout group) that also contains some of the neighboring structures.(to give the proper constraints and do a breakout)
-Extract the freebody loads asking for applied, reaction, multipoint reaction and peripheral elements. This is done to ensure that you have the correct boundary conditions.
- Create one fixed constraint at a sturdy structure away from your structure.lets call this breakout constraint
-Create another set to constrain all of the nodes in your aset group.
-Add the loads using model>loads>loads from freebody
-run your analysis using the constraint sets and ask for slightly negative eigenvalues(sometimes positive small numbers cause stability problems)
-Analyze using the one point breakout constraint and the ASEt set as your asset set to get your buckling results.

I hope this helps. Cheers.

ps. Namklof: the run times don't and didn't change with the solver and the sturm method actually had problems running for certain ranges for some unbeknownst reason(maybe range was too big).Lanzclos seems to work fine. Nonetheles, it was a good exercise to validate my results.

ps2. a good resource: [URL unfurl="true"]https://femci.gsfc.nasa.gov/eigenmethods/index.html[/url]