Hi everyone. I'm working on a modal analysis of a thin cylindrical shell using different programs to make a comparison of the natural frequencies, in particular Abaqus/CAE , Nastran In Cad and Mathematica. I've made the model in Nastran and have calculated the frequencies, and have made the same model (geometry and properties) in abaqus but the results of the two programs don't match. So I wonder if it is a problem of discretization /mesh. In this case can I export the Nastran model, completely included the mesh, in abaqus and than run the frequency analysis using the nastran file? If yes, in which way?
Please, share your Nastran model. You might want to use meshio to convert the mesh. https://github.com/nschloe/meshio
Problem solved, I think. I exported the nastran input file into Abaqus, and the model complete with mesh appeared on my abaqus desk, than I applied the boundary conditions and create a set (linear perturbation --> frequency). After that I create a Job and made it run. Now the mode shapes and the corresponding frequencies are the same with an error of at most 0.5%.
But I really can't understand why if I create the same model from scratch in Abaqus the frequencies and the mode shapes are too different compared to nastran frequencies.
You can compare both inp files (for imported model and created from scratch one).
Hi
Perhaps any of this is useful?
https://www.nafems.org/publications/resource_center/p18/
Presentation Analysis Technology:; A discussion on some of the fundamentals
NAFEMS has been barking up this tree for quite some time.
As you can see in the above presentation, running one and the same model through different FE software produces different results, so much so, that after 10-15 modes the computed mode shapes are the more different than they are alike.
I always thought this to lie in the difference between element formulations. However, one forum member stated that it has been shown very much to depend on the solver that is used.
My only experience on solver dependency was when the Nastran complex mode solver was first released. Then, you got different results running the same input deck with the exact same settings. When asking support, I received the reply that - computing complex modes is a hobby for gentlemen. This feature disappeared in the next release.
So - you might want to toy also with solvers and solver tolerance settings to see what happens? Please share your findings - this topic is fun.
Thanks for the interest Claes Richard Fredö . If you followed the discussion I have come to have a perfect match between the Abaqus results and Nastran results, but only with the imported Nastran input file that I ran in Abaqus. Then I compared the two Abaqus files: the one made from scratch and the one imported, and there it is! I noticed that in the file imported from Nastran there were different element types, in particularly S8R and some triangular elements which I can’t remember the name, but in the file made from scratch in Abaqus there were only linear quad elements: S4R. Thus I made a new model in Abaqus with the same elements of Nastran file (parabolic order) and ran again. The results were perfect. It was a simply elements definition problem!
Hi
A flat plate is one thing. We even managed to get perfect match between Test and FE for this.
Try adding some other types of elements & element orders and at an angle for the fun to start.
- Badges
- Science topic