October 17, 2023 at 9:25 amPanagiotisSubscriber
When trying to mesh a cylindrical tank with heads close to elliptical shape ( it is not a half ellipsoid) I get the following error "The mesher has detected a discontinuity in the model and is unable to handle it. Please go back to the CAD system and correct the model." The problematic geometry is shown in the picture (with red dots). Although I have checked the geometry in spaceclaim and have already clicked the share topology option, I keep getting this error. The geometry in spaceclaim is comprised of multiple solids and was generated through the revolution of an area through the z-axis.
P.S. I have already meshed the same geometry in Mechanical APDL, using APDL commands and not spaceclaim. However, I want to make the transition from APDL to Workbench, in order to add other features to the CAD file.
October 18, 2023 at 2:15 pmGovindan NagappanAnsys Employee
Inspect the probelmatic geometry and see if you can correct it?
In Mechanical, you have tools to display edges in different colors based on connectivity. (Color -> By connection). See if it helps to identify the problem. If there is a gap larger than the tolerance, shared topology may not have connected the geometry at this location. See if you can fix the gap in spaceclaim
If you have access to meshing, you can consider meshing in Spaceclaim using blocking
Or try a different method and see if it helps. Try patch independent methods like Multizone for hex meshing or patch independent tetrahedron
Default is patch conforming methods in Mechanical (PC tetra and Sweep). These methods require a propely connected geometry. So, other methods may help. in MAPDL, you can create 2D mesh and sweep. We have similar tools in newer versions f Mechanical - Check this link: Pull (ansys.com)
See if these tools help
October 18, 2023 at 3:11 pmmjmiddleAnsys Employee
When you select "Show Problematic Geometry" on an error message, the red dots do not usually show an exact problem location. Instead, the red dots are just the highlighted vertices of green highlighted faces. You should ignore the red dots and inspect the green highlighted faces. Zoom in close and insect the face boundaries especially.
Also, the defeature tolerance in the global mesh object can overcome geometry problems. Make sure it is turned on and you should estimate a reasonable distance to merge across. Try specifiying a larger tolerance.
The share topology in SpaceClaim can cause corruptions in the geometry if you set up sharing, and then make further modeling changes. It should be done as one of the last things in SpaceClaim. You can delete all share topology and redo the sharing. Also, you should test by completely removing all shared topology and see if that meshes in Mechanical. That will at least tell you if the shared topology is the cause.
- 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
- 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
- Defining rigid body and contact
- Colors and Mesh Display
- A solver pivot warning or error has been detected
© 2023 Copyright ANSYS, Inc. All rights reserved.