Learning Forum

[rkoomul]

 Hi,

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

Thank you

 

[Sandeep Medikonda]

Have you tried share topology in SpaceClaim or Design Modeler? If not, please see how to do this in these videos:

Regards,
Sandeep

[rkoomul]

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.

Thank you,

Roy

 

[Karthik R]

Hello Roy,

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.

Thank you.

Best Regards,

Karthik

[rkoomul]

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?

Thank you,

Roy 

[Karthik R]

Hello Roy,

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.

Best Regards,

Karthik