Is it possible to run a modal analysis with non-linear connectors?

[flyforever85]

I ran a modal analysis of a tower with guy-wires modeled by non-linear connectors (no compression only). I received a critique that the modal analysis doesn't give a correct answer since the presence of the non linearity but no other feed back. Can someone tell me what would be the problem?

 

[FEA way]

Eigenfrequency extraction is a procedure meant for models with linear behavior. The closest you can get is complex eigenvalue extraction analysis. This one can include some forms of nonlinearity.

 

[mgriebel]

Running a modal analysis of a nonlinear model will linearize the model. If you have nonlinear elements or material definitions, it will use the current configuration as the reference configuration for the modal analysis. If your nonlinear connectors are preloaded before the modal analysis, they will remain in tension during the modal analysis. If there is no preload step, I'm uncertain how they would respond. I'd lean towards them being in tension (i.e. having stiffness), but I would test to confirm.

 

[flyforever85]

THank you.
I guess my model doesn't include the guy-wires simply because the frequency with and without them is pretty identical. There is no pre laod for any of them, they just generate a force along their length if displacements are positive e no force at all if displacements are negative. I was suggested to first load the tower in order to put in tension some of the guy wires and then run a modal analysis on that new configuration. Any idea how to do that?

 

[FEA way]

Indeed, you can load the tower in general static step preceding modal analysis and then use natural frequency extraction procedure to evaluate modal response of now prestressed structure.

 

[flyforever85]

In the past I remember having a model that I used to analyze for both stress and modal. And if by chance I had both steps active the analysis would freeze: literally it would show submitted and nothing else. I'll give it another try, but I'm also trying another approach. from the stress step I obtained the displacements due to a certain load and now I'm imposing the same displacements as boundary conditions in the modal analysis

 

[mgriebel]

If you perform a modal analysis following a general static analysis step, the initial stress and load stiffness effects will only be accounted for if geometric nonlinearity was accounted for in the preceding step. If geometric nonlinearity is not accounted for, the stiffness matrix is never updated, and the modal analysis will consider the base state as the undeformed state when the stiffness matrix was last calculated.

 

[FEA way]

Maybe that model in the past was large and caused performance issues. Anyway, prestressed modal analysis is pretty common technique. Check the documentation chapter "General and linear perturbation procedures" (Abaqus Analysis User's Guide) for more details.

 

[flyforever85]

Thank you both for the help. Apparently the modal analysis works after a step only if Lanczos is selected. For this model (and the previous I mentioned) I selected AMS as a solver and that didn't work. Try yourself if you'd like!

 

[FEA way]

Did you get any error message ? AMS eigensolver has some limitations (for example it doesn't support piezoeletric elements) but it should be possible to perform prestressed modal analysis with it. Lanczos is default choice while AMS is recommended for large models with large number of requested eigenvalues.