Hybrid meshing in ICEM for 2D conjugate heat trnasfer
 

Hello,
I want to simulate a 2D conjugate heat transfer set up in Fluent and I am making the mesh in ICEM for that. A simplified model of my setup is shown in the attached picture.


The rectangular block is a solid with two rectangular holes in it. At the inner edges of the block a fixed temperature would be given and from those edges, conduction will occur to the outer edge of the block. From that outer edge, convection will occur to the surrounding flow.



I want to make a structured mesh around the block with the usual blocking approach and I intend to have a coarse tet mesh inside the solid block. If I have understood what’s given in the Fluent manual well, the mesh in the hollow solid cylinder can be coarse. However, the usual boundary layer resolution would be required around the outer edge.


My question is, how I can make a tet mesh inside the solid block and structured blocked hex mesh around the block in ICEM?



I have tried to surface mesh the solid block but it gives a weird mesh. I can of course split the block and associate edges and curves to the holes, but this will be a mess since there will also be an O-grid around the solid block. Another method I tried was to make the block for the solid a free type. Since, this block was not split and not associated with the hole edges, the block just covers the entire rectangle without capturing the holes.

http://i67.tinypic.com/2vbsit5.jpg
http://de.tinypic.com/view.php?pic=2...9#.WqlJzufA-Uk
http://de.tinypic.com/view.php?pic=2...9#.WqlJzufA-Uk

Hi Ishan,

do you have access to the tutorials coming with icem? If not, google is your friend: https://www.sharcnet.ca/Software/Ans...t/icm_tut.html

There is a tutorial creating a hybrid mesh.
Search for "Merged Tetra-Hexa Mesh in a Hybrid Tube"

Best regards,
Sebastian

Hi Sebastian,

Thanks for pointing to that tutorial. Unfortunately, I don't have acess to tutorial files. I never had. But yes, I will look into it. My bad as I overlooked the primary source of help. I rarely, look into those tutorials since I don't have acess to the files used in them. I usually try looking deeper into the Help/User manual of ICEM or YouTube.

Regards,
Ishan

Official ICEM tutorial files are included in your installation. There should be a sample/CFD_tutorial subfolder in your ICEM installation directory where you can find them.

Hi Kad and hello again Sebastian,

Thanks for bringing that to notice, but I can't seem to find the files in my installation. However, I got it from one of my colleagues.

Regarding my meshing, I have a question. The hex-tet mesh tutorial was somewhat useful in the sense that I got to know about the merge meshes feature. But that feature is only for 3D meshes. To workaround that problem, I have decide to go with non-conformal meshes which can be made into interfaces in Fluent.

In my geometry, I have been sucessful in creating a tet mesh inside the rectangular block. Hex mesh in the air domain was not an issue and I can do that again.

I have two sets of curves from where the CHT will occur; rectangle and air. The idea is that, I will make an interface between these two curves and give the coupled wall in Fluent. However, I am not able to undertsand how should I import this mesh into Fluent.

I tried to follow this thread's suggestion of importing the mesh from the solid and air domains separately and them making and interface but that doesn't seem to work because the TUI oiptions are missing:

https://www.cfd-online.com/Forums/an...hexa-mesh.html

Addituionally, I have been trying to play around with the "merge nodes" feature but that hasn't helped much.

Any info on importing the mesh or making the conformal mesh in 2D would be helpful.

Creating interface between two separate non-conformal meshes in fluent:
Load the first mesh. Load the second mesh by going to Mesh->Zone-> Append Case File. Then change the boundary conditons for the interface walls to ->interface. Having done that you can create a coupled interface under Define -> Mesh interface.

Conformal 2D hybrid mesh:
Start with hex mesh for the outer region. Convert blocking to unstructured mesh and make shure to have the "line elements" available. Line elements are created automatically on all curves that have edges (blocking) associated to them. Pick patch dependent All-Tri mesh method for the unstructured part. Now turn on the option "respect line elements" under shell meshing parameters. This option forces the tri mesh to align with the existing line elements and it creates a conformal mesh. I have made a little example with the option turned on/off.

Hi,
Thanks for the info and the images showcasing the method but this is exactly what I have been trying for quite a while. I made my own simple geometry somewhat similar to what you have made. I want a conformal mesh between the edges named „air_inner“ and „solid_outer“.
So, I made a geometry somewhat similar to what you have. I have attached the pictures of it.

1. I first made the hex mesh for the „outer air domain“
2. Converted it to unstructured mesh
3. To make just the tet mesh inside the solid, I first made a material point for the „solid“ domain
4. After I made the material point for „solid“, I gave the part meshing sizes just for „solid“
5. Then, I chose the All-Tri mesh type with Patch Dependent method, respecting the line elements with ignoring the size of 0.001 ( not sure what does it do)

7. After this, I generate a surface mesh for „solid“

But, now I have another problem. Whenever I generate the tet mesh, the unstructured hex mesh just disappears even though the mesh tab is checked on. Am I doing something wrong here or is it a bug, I am not sure. But, the desired mesh just doesn't generate.


https://preview.ibb.co/gkJehx/air.png


https://preview.ibb.co/kHrApc/solid.png

Maybe you are doing something wrong when generating unstructured tri mesh.

As a hint in general, material points have no meaning in 2D. They are only relevant for 3D meshing. The 2D interior mesh is assigned to the surface part that it is created on (for unstructured tri). In 3D materials points mark a closed volume and the interior mesh is assigned to the part of the material point. But again, in 2D it does nothing. So in your case, you should name the inner solid surface ti something like SOLID.

When computing the unstructured surface mesh you have to specify the correct input. As you only want to mesh the very inner surface, this surface is the only input for mesh generation. Under Compute surface Mesh choose Input -> from screen and pick only the SOLID surface. Now generate the tri mesh.