May 23, 2022 at 9:23 amshiva.maheshwariSubscriberI 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
May 23, 2022 at 12:28 pmAniketAnsys EmployeeAnsys 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.
How to access Ansys help links
Guidelines for Posting on Ansys Learning Forum
May 23, 2022 at 12:38 pmpeteroznewmanSubscriberModal 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.
May 23, 2022 at 2:06 pmshiva.maheshwariSubscriberThanks 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?
May 23, 2022 at 3:56 pmpeteroznewmanSubscriberThe 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.
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- whether have the difference between using contact and target bodies
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
- Colors and Mesh Display
- material damping and modal analysis
© 2023 Copyright ANSYS, Inc. All rights reserved.