September 17, 2020 at 7:41 pmCheta RathodAnsys Employee
This could be due to the bonded contacts with large gaps present in the Modal analysis. Gap/Penetration at bonded contact adds extra stiffness to the model in Modal Analysis when the contact formulation is set to program controlled (penalty method).
Background: With large gaps, Bonded contacts using penalty methods can have accuracy issues. There is a warning issued for the user to either clean-up the model using cnch.adjust or morph or switch to MPC.
Warning message from the output is copied below.
**WARNING*: The initial penetration/gap is relatively large. Bonded/no separation option may cause an accuracy issue. Switch to MPC algorithm or you may use the CNCHECK,ADJUST/MORPH command to move the contact nodes towards the target surface.
Resolution: Change the bonded contact formulation with these warnings to MPC formulation. This should give zero frequency modes for the unconstrained DOFs. As a check, compare higher frequency modes using both MPC and penalty contact formulations. There should be minor changes in the higher frequencies for the same mode shapes.September 21, 2020 at 12:07 pmSeptember 24, 2020 at 4:30 pmDave LoomanAnsys EmployeeThis issue only affects the rigid body rotational modes. The penalty based contact across an open gap acts like a rotational constraint.
Viewing 2 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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.Trending discussions
- How to calculate the residual stress on a coating by Vickers indentation?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- whether have the difference between using contact and target bodies
- Colors and Mesh Display
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- Massive amount of memory (RAM) required for solve
- What is the difference between bonded contact region and fixed joint
Top Rated Tags
© 2022 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.