January 27, 2021 at 10:19 pmenina1992Subscriber
I am trying to emulate the picture below by imposing symmetric boundary conditions so that I can improve my mesh size by reducing the geometry.January 27, 2021 at 11:24 pmpeteroznewmanSubscribernThank you for fully documenting your question, it makes it easy to give you guidance.nThe shaft is bending up, so you can only use two planes of symmetry, a vertical one through the center of the wheel, and a vertical one through the axle. Because the axle is bending up, you can't slice horizontally through the axle. You haven't shown a triad, so I don't know which direction is up, but I will assume it is the Y axis.nYou either use Symmetry Regions or you use Displacement supports, you don't do both because they each do the same thing, but if you did both correctly, it wouldn't hurt, it is just a waste of time setting it up.nBut you have a mistake in two of the symmetry regions. The Symmetry region Details window has a Symmetry Normal setting and its default value is X axis and that doesn't automatically change when you pick the faces, you have to manually match the Symmetry Normal and type in the correct normal, such as Y and Z. However, you only want two planes, X and Z and you don't want a Symmetry Region for Y, as that is the horizontal plane.nThere is a better constraint than Fixed Support for the end of the axle. Delete that. Delete the two Displacements and use the two corrected Symmetry Regions. Those take away 5 degrees of freedom of the wheel. The last constraint is in the Y direction. Put a Remote Displacement on the end face of the axle where you had the Fixed Support. Now you can leave everything Free except put a 0 for Y.nIf the total force on the full model was F, then you apply F/4 because you only have 1/4 of the model when you make two vertical cuts. nViewing 1 reply thread
Ansys Innovation Space
- 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.Trending discussions
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- 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
- User manual
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- material damping and modal analysis
- Colors and Mesh Display
Top Rated Tags
© 2023 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.