March 30, 2023 at 2:22 pmDiego MolinaSubscriber
hello! I'm having trouble meshing a part with multiple bodies. What I'm trying to do is a static simulation for a vertical storage tank, it's made up of 5 rings (different thickness, so I use 5 different bodies) and the roof (also multiple bodies). When using adaptive mesh size, the mesh in the tank shell is extremely strange (attached screenshot), not using it improves the mesh, but I cannot reach convergence because making the elements smaller is too much computational load (for this I require use adaptive size)
I have tried:
1. Use shared topology
2. Use edge/edge and face/edge automatic contacts
3. Using a single body on the rings (improves, but I can't assign different thicknesses this way)
4. Turn off/on "defeaturing"
What workflow do you recommend to solve this problem?
April 1, 2023 at 5:11 ammjmiddleAnsys Employee
The elements are very small throughout the model. This will increase solution time a lot. Why are they so small? Is this outer body very thin? The strange patchs of mesh may be affected by nearby fearures on the faces on the other side. If this is a thin body, it is usually better to make midsurfaces in the CAD modeler, which have thickness assigned. This will allow larger element sizes; the solution will run faster, and convergence should be easier. Set "shell thickness effect" on contacts used to connect bodies, and be sure to specify the correct "top" or "bottom" on "contect shell face" for contact and target side selections.
Also, consider specifying a larger element size on the global mesh object, setting refinement back to 1 and creating local mesh size features under the global Mesh object. For these you can just select faces/edges where you want the element size smaller.
Also consider turning off the adaptive mesh size function. Turn "Capture Curvature" on and set a minimum size for the curvature. Also set appropriate max mesh size and general element size throughout most of the model..
April 3, 2023 at 9:31 pmDiego MolinaSubscriber
It worked! Thank you so much, I'm using surfaces. I turned of the adaptive mesh size function and turned un capture curvature, and set local mesh sizes for the rings and the roof components, now i am getting some stress peaks at the border of some bodies, is this due to the meshing process or is due to the geometry?
April 3, 2023 at 4:45 amsaas lamaSubscriber
It is possible to create local mesh size features below the global Mesh object by providing a bigger element size on the global mesh object, resetting the refinement level to 1, and doing so. In this case, all you have to do is choose the faces or edges where you want the element size to be reduced.
April 4, 2023 at 1:04 pmmjmiddleAnsys Employee
The location(s) in the first picture look like typical stress singularities. Set smaller mesh sizes in the location of the max stress. If successive solutions with smaller mesh sizes cause the max stress to increase at increasing rate, it is a stress singularity. Valid max stress values will approach a constant value asymptotically with successive solutions using smaller mesh size. Stress singularities occur at corners. If the region is not of interest just scope results away from these. If it is a region of interest, make small fillets/rounds at those locations and use a small enough mesh size to model the round.
June 1, 2023 at 1:08 pmRouzman DallinSubscriber
Hello, This subject very interesting. thanks for helpfull writing. this article very important and true.
thanks for helpfull writing. this article very important and true.
- 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.
- 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
© 2023 Copyright ANSYS, Inc. All rights reserved.