Learning Forum

[shiva.maheshwari]

I have performed a Modal Analysis on a assembly . But in results at some high frequencies there are some inconsistent results.
The outer casing of assembly crossing the inner bodies without deforming them .
Is it due to contact definition or some other reason?
Does mode results are reliable in this case or not?
How could I resolve this issue?
I have attached images for reference

[Aniket]

Ansys staff can not download any files on the forum, so if you want to reach a larger audience to get answers, please insert inline images describing your problem. (1.jpg and 2.jpg)
But from the looks of it from the inline images, you are doing a modal analysis. And some modes have bodies passing through each other. First of all, the modal analysis is a linear analysis, so it treats all contacts at their initial configuration. Meaning even if you have a nonlinear contact such as frictionless or frictional, it will check the initial contact status, and if the contact is open initially, there will be no interaction between the two bodies at all.
So insert a contact tool under contact and check the initial status of all the contacts, if you feel any of the contacts are open initially and should be closed take corrective actions such as increasing pinball radius, making the contact adjust to touch, etc and rerun the modal.
Please note that even if a nonlinear contact such as frictional is closed initially, it will not be free to slide while doing modal and will be treated as bonded.
-Aniket
How to access Ansys help links
Guidelines for Posting on Ansys Learning Forum

[peteroznewman]

Modal is a linear analysis so nonlinear contact is not permitted in the analysis. When nonlinear contact is in a model and works in a Static Structural analysis, Mechanical will automatically convert nonlinear contact to bonded contact if the initial contact status is closed, or it will ignore the nonlinear contact if the initial contact status is not closed, when a Modal analysis is requested.

[shiva.maheshwari]

Thanks peter
So it means I can ignore those deformations and the modal frequency I am getting are correct .Is it?

Also I tried giving contact(frictionless) b/w those two surfaces but it was changing the output modal frequencies.
As Initially there is no contact. So, Is it right to give contact in b/w them?

[peteroznewman]

The magnitude of the deformation is arbitrary in a Modal analysis because there is no applied load. It is just showing you the mode shape and frequency. If you do Harmonic Response, then you are applying a load and the deformation is real.
Frictionless contact is a Linear contact so will be used in a Modal analysis and will result in the frequencies changing from a Frictionless contact if the contact is closed.
If there is a gap between the two panels, then the correct condition is no contact. You can evaluate if there will always be a gap when you run other analyses.