November 8, 2018 at 11:45 pmrkoomulSubscriber
I am trying to get a matched surface mesh at an interface between two different bodies and not able to get it working. This is to simulate heat transfer from molten metal to a crucible. I created the geometry as two parts, with one body in each part, in the design modeler. When I brought it to Meshing, I am able to get the correct interface under "Connections -> Contacts". But, when I generated the mesh, the surface meshes on those two bodies are different. Therefore, there are some gaps between the meshes (see the attached images). How do I get a matched surface mesh at the interface? I tried inserting "Mesh -> Insert -> Contact Match". But it didn't help.
I am using Version 19.1
November 9, 2018 at 1:21 amSandeep MedikondaAnsys Employee
Have you tried share topology in SpaceClaim or Design Modeler? If not, please see how to do this in these videos:
November 9, 2018 at 3:04 pmrkoomulSubscriber
Thank you Sandeep for the reply. I tried shared topology from DesignModeler. To use the shared topology, I included all the bodies under one part. Then the mesher created matched mesh on the interface. But, I am not getting interfaces under "Connections -> Contacts". I tried to create the interfaces using "Create Automatic Connections" and "insert -> Manual Contact Region". Both didn't work. For the manual connections, it is not accepting the surfaces for "Contact" and "Target". Without interface setup, I am not able to set proper boundary condition inside Fluent. That is the reason why I tried to keep the bodies under different parts. When I keep the bodies under different parts, I am able to get proper interfaces, but not able to get matched surface meshes.
November 13, 2018 at 11:00 pmKarthik RAdministrator
Using Sandeep suggestions, you will not have interfaces in your model. However, it will help you create a conformal mesh on all your geometry.
If you need interfaces, I'd suggest you keep your bodies as separate objects (an not as a single part). You will see interfaces in this case. You can select the surface that form an interface and insert a face sizing on these surfaces. This will allow you to keep similar sizing on both these surfaces. However, this will not be able help you create a conformal grid.
Please let us know if this helps.
November 13, 2018 at 11:14 pmrkoomulSubscriber
Thank you Karthik. Which approach do you suggest if I have to simulate heat transfer from a fluid domain to a solid domain? 1) Keep both bodies in one part and get a conformal mesh or 2) Keep both bodies in separate parts and get a non-conformal mesh, but a mesh with an interface. If it is the first approach, how do I specify the boundary conditions at the interface between the domains? Also, do I need to create interfaces to apply boundary conditions? If it is the second case, will the small gaps between non-conformal meshes create any issues. Do you have any tutorial on any similar problem?
November 13, 2018 at 11:30 pmKarthik RAdministrator
You can use either approaches.
In the first approach, you will have to use manually couple the interfaces. Please see the video below.
I'd prefer using a conformal mesh approach. In this approach, Fluent would automatically recognize the solid-fluid interfaces and assign what are called 'wall' and 'wall-shadows'. You can use the thermally 'Coupled' wall boundary condition to model the heat transfer. This boundary condition would show up as soon as you read your mesh into Fluent and enable 'Energy equation'.
Please check out the following example on conjugate heat transfer. I hope this helps.
With interfaces - non conformal mesh
Without interfaces - conformal mesh
In the second video, they do not show the coupled wall BC. But if you click on either the wall or its shadow, you should have a coupled wall boundary condition automatically.
I hope this helps.
- You must be logged in to reply to this topic.
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.
- ANSYS Workbench Measuring within Design
- how to improve the inflation quality at sharp corners?
- check element type
- The mesh file exporter could not resolve cyclic dependencies in overlapping contact regions error
- How to resolve Mesh Failure
- Meshing Error
- Error in meshing
- Conformal vs Non-Conformal Mesh
- execution error inside the mesher. The process suffered an unhandled exception or ran out of memory
- inflation created stairstep mesh at some location
© 2023 Copyright ANSYS, Inc. All rights reserved.