modal analysis with contact boundary condition

Hi,there.

It seems that ANSYS doesn't provide modal analysis with contact boundary condition(structure-structure contact).

Please recommend any FEA software which can do the job.

Thanks in advance.

"ontheway" wrote in news: snipped-for-privacy@f14g2000cwb.googlegroups.com:

Modal analysis assumes a linear system. Contact problems are non linear. So, you can't do a modal analysis in the presence of contact (well, you can in practice, by linearising the non linearity).

You are probably trying to do something more like dynamic analysis, which of course ANSYS will do just fine.

Cheers

Greg Locock

What engineering problem do you want to solve? Do you want to use mode superposition to reduce the calculation time? The latter is actually possible, at least for the nodal contact, when you treat the contact as nonlinear input.

Best wishes,

Evgenii Rudnyi

--

This situation requires a nonlinear modal analysis solution. A simplified way to handle this would be replacing contact elements with springs.

Ansys can do nonlinear transient (dynamics) analysis.

like there should be a way to do nonlinear modal analysis.

Nastran and Abaqus both have nonlinear modal analysis solutions in one way or another.

The problem that I am tacking is ...

Free vibration of thin plate deformed by cylinder

First, a thin cantilerver plate undergo large deformation by contact with rigid cylinder surface. (static analysis)

Then I'd like to extract 'resonat frequency' of the thin plate if there is any.

I know that it's nonlinear problem but don't you think there is resonant frequency, do you?

The problem that I am tackling is ...

Free vibration of a thin plate deformed by cylinder surface

First, a thin cantilerver plate undergoes large deformation by contact with rigid cylinder surface. (static analysis)

Then I'd like to extract 'resonant frequencis' of the plate in contact with the cylinder surface if there is any.

I know that it's a nonlinear problem but don't you think there are resonant frequencies, do you?

In ANSYS, there is a prestressed modal analysis. That is, first you deform the plate, then you determine resonant frequencies for the deformed plate. They are different then those for the original configuration. It well may be that you can use this technique.

Best wishes,

Evgenii Rudnyi

--

However the prestressed modal analysis provided in ANSYS does not allow contact boundary condition.

It reads "Modal analysis in the ANSYS family of products is a linear analysis. Any nonlinearities, such as plasticity and contact (gap) elements, are ignored even if they are defined." in 3.2. Uses for Modal Analysis of Structural Guide.

seems to me you need to force the model to do what you want.

use the 'prestressed modal analysis" but eliminate teh contact element; replace it with a suitable spring or a rigid support whichever suits your situation best.

cheers Bob

Yes and no.

1) Yes, model analysis is linear. Well, you can include damping that makes it in some respect nonlinear as well. It is clearly depend on how you define nonlinear modal analysis. It may be good if you do it.

2) Calculation of the prestress is nonlinear. You can include large deformation. Actually, I do not know about contacts but why not. The prestressed effects is within the stress stiffening matrix. The question is if it includes the effect of the contact. Presumbaly, it should.

You see, you should first express your problem as a mathematical problem. After all, simulation is a numerical solution of some mathematical problem. Whether a particular software can handle this, it is another problem. At present, I do not quite understand a mathematical problem that you would like to solve.

Best wishes, Evgenii Rudnyi

--

de/simulation/mor4ansys/

I'm not well-versed in it, but many of my co-workers recommend DYNA for contact modeling. We generally use NASTRAN, but sometimes use DYNA when we need to model some sort of contact. (NASTRAN isn't that great for contact modeling)