Patran/Nastran Buckling Help - Please

[Burner2k]

OK folks,
After a lot of attempts, I'm unable to solve a simple 1D nonlinear column buckling in MSC Nastran. I can do the same in Femap (Sol 106) and get reasonably good agreement between hand calc & SOL 105 results. But with Patran/MSC Nastran, I can run the solution in SOL 106, the buckling load is 15% higher and deformation mode shape doesn't make sense.

I have to point out here that my column is "long" i.e. the buckling domain falls in elastic region and thus Euler's formula should hold good.

I have tried Googling for any papers, literature and materials in which, the actual FEM procedure of either SOL 106 or 400 of column nonlinear buckling has been provided, but I nothing turned up. It just could be that I am not very good at research.

I have an I Section; simply supported at ends. FE representation is via CBEAM elements. A small moment is applied to induce the initial imperfection and a compressive load of 100,000 lbs is applied.

I would appreciate some help. I know this site is meant to provide tips not complete procedures, but if some could provide a dat file of a successful analysis, I would be immensely thankful.

I will post the dat/bdf files of my model if required.

 

[Burner2k]

Answering my own topic.

I was able to obtain reasonably satisfactory inelastic column buckling results with Patran as well.

The critical buckling load per my hand calc (& Bruhn) is around 15500 lbs. I am getting some where between 16000 & 17000 lbs (the analysis stops converging at load step 0.17 out of 100) and the corresponding crit stress is close to 31.8ksi. Not too far off.

Perhaps if I play a little bit more with initial imperfection, I may be able to get more accurate values.

A point of note on how to capture the Eigenvector mode shape from SOL105 and use it as initial imperfection in Nonlinear Analysis.

Step 1: Plot the Marker->Vector of Eigenvector

Step 2: Create a Field->Spatial->FEM
In this, choose vector option. Choose the group in the "groups tab" and click on options. In options, I chose Linear Extrapolation from the drop down menu. I reckon choosing "Closet Tabular Value" should work as well!

Step 3: Under Utilities -> FEM Nodes -> Move Nodes by Field -> Select Offset, enter offset value, select the above created spatial field and finally select the nodes which are needed to be offset.

I chose an offset value of 0.01 for the above case.

I hope the above helps.

Apparently, the offset can be accomplished using Result->Result->Combine->Eigenvector Deformation command (will create a new subcase). But I could not find any way to associate the above combined subcase to nodes offset/move.

If folks are familiar, please help out.

 

[ESPcomposites]

For long columns, the solution is relatively insensitive to the initial imperfection. This is because the stresses rapidly increase as a function of the load when the the load is near the critical load (i.e. bifurcation problem). If I remember correct, these can usually be predicted to within a few percent of the Euler solution.

For short/intermediate columns (more practical problems), the result is more sensitive to the initial imperfection. With some rules of thumb and experience, you can predict these within reason. But you may not be able to predict to within a 5% percent across the entire range of intermediate lengths. I suppose you could back calculate some values to determine the most effective way to apply the eccentricity. I have tried a few different approaches and it works good enough.

Brian

http://www.espcomposites.com