[hz283]

Hi All,

Now I had a problem about how to deal with the "interface" or "interior" faces in Openfoam.

The Problem is like this:
I used ICEM to generate the meshes. Since the computational domain is complex and so I divided into the domain into several bodies. I generated the meshes for each body and then merge them together. Since the nodes belonging to the two neighboring bodies are not matched. I used "move nodes" to make them coincide. I tested this method using fluent and it seemed it is OK. But this mesh is read by Openfoam, the error message is like this:

Cannot find metach for first face. cell model: tet first model face 3(1 2 3) mesh face:
4
(
.....
...
...
...
)

I also tried the mesh with the interface nodes not moved by "move nodes" and this error does not appear.

I have tried to get some solutions for this:
1, try to improve the mesh using ICEM ? (using this method means that I should make the nodes on the interface metached from two sides)
2, using AMI to deal with the non-conformal mesh ? I checked the tutorials (http://www.openfoam.org/version2.1.0/ami.php) for AMI, but I found there is always another file about topoSet. Is this file particularly for AMI? (using this method means that it is not necessary to make the nodes matched.)

I think the interface or interior face between different bodies or mesh regions are common. But I do not know which method is the best way for Openfoam ? Does anybody know something about this? Any suggestions and comments are
welcome!

best regards,
H

[hz283]

Hi All,

Does anybody know something about this?

best regards,
H

Originally Posted by hz283

Hi All,

Now I had a problem about how to deal with the "interface" or "interior" faces in Openfoam.

The Problem is like this:
I used ICEM to generate the meshes. Since the computational domain is complex and so I divided into the domain into several bodies. I generated the meshes for each body and then merge them together. Since the nodes belonging to the two neighboring bodies are not matched. I used "move nodes" to make them coincide. I tested this method using fluent and it seemed it is OK. But this mesh is read by Openfoam, the error message is like this:

Cannot find metach for first face. cell model: tet first model face 3(1 2 3) mesh face:
4
(
.....
...
...
...
)

I also tried the mesh with the interface nodes not moved by "move nodes" and this error does not appear.

I have tried to get some solutions for this:
1, try to improve the mesh using ICEM ? (using this method means that I should make the nodes on the interface metached from two sides)
2, using AMI to deal with the non-conformal mesh ? I checked the tutorials (http://www.openfoam.org/version2.1.0/ami.php) for AMI, but I found there is always another file about topoSet. Is this file particularly for AMI? (using this method means that it is not necessary to make the nodes matched.)

I think the interface or interior face between different bodies or mesh regions are common. But I do not know which method is the best way for Openfoam ? Does anybody know something about this? Any suggestions and comments are
welcome!

best regards,
H

[wyldckat]

Greetings hz283,

I've moved your thread to the sub-forum that is dedicated for other meshers and OpenFOAM. You can find the sub-forum by going to:

• OpenFOAM Meshing & Mesh Conversion
  • OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ...

On this sub-forum you can find the following threads :

• http://www.cfd-online.com/Forums/ope...-openfoam.html
• http://www.cfd-online.com/Forums/ope...tml#post346373

Hopefully those two threads can provide the information you are looking for.

If not, I suggest that you create a simple test case that shows the problem you're having and share it with us, so that it's easier to help you find the solution with some trial-and-error.

Best regards,
Bruno

[hz283]

Hi Bruno,

Actually I have done the test using the a backstep by ICEM.

I divided the whole computational domain into three bodies: nozzle, step and exit. There are two interfaces between nozzle and step, step and exit, respectively. And then I generate the mesh body by body, then merge them in ICEM.

I tried two methods:
1,in ICEM, I make the grid nodes from two bodies matched. Then output the mesh and set the interface face to be "interior", output the fluent format mesh. I used fluent to read the mesh. It is OK, but it is not when I used Openfoam.

2, I did not make the grid nodes matched and then output the fluent format mesh. The openfoam can read in without any error (I did not run it) but fluent will show errors.

I can share my fluent format mesh but I do not know how to upload it.

Thank you.
H

Originally Posted by wyldckat

Greetings hz283,

I've moved your thread to the sub-forum that is dedicated for other meshers and OpenFOAM. You can find the sub-forum by going to:

• OpenFOAM Meshing & Mesh Conversion
  • OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ...

On this sub-forum you can find the following threads :

• http://www.cfd-online.com/Forums/ope...-openfoam.html
• http://www.cfd-online.com/Forums/ope...tml#post346373

Hopefully those two threads can provide the information you are looking for.

If not, I suggest that you create a simple test case that shows the problem you're having and share it with us, so that it's easier to help you find the solution with some trial-and-error.

Best regards,
Bruno

[wyldckat]

Originally Posted by hz283

I can share my fluent format mesh but I do not know how to upload it.

Since I've got a feeling that your mesh is larger than 100 kB, I suggest you try Dropbox: https://www.dropbox.com - or it can be any other file sharing
website. All of the big companies now have it... some examples:

• Google Drive
• Microsoft SkyDrive

[hz283]

Thank you so much, Bruno!

Just now I think I found that solution:

For multi-body meshes from ICEM, we can merge the grid nodes from two bodies at the interface face and then use the command fluent3DMeshToFoam.

But I am not sure if the following method can work or not:
Do not merge the mesh nodes at the interfaces and then AMI in openfoam.

Any comments are welcome.

Thank you again.
H

Originally Posted by wyldckat

Since I've got a feeling that your mesh is larger than 100 kB, I suggest you try Dropbox: https://www.dropbox.com - or it can be any other file sharing
website. All of the big companies now have it... some examples:

• Google Drive
• Microsoft SkyDrive

[Miner]

This sounds a lot like a problem I have. I made a Fluent mesh and imported it using Fluent3DMeshToFoam. That worked fine. But I have a conjugate heat transfer problem, and if I make the fluid and solid meshes from 2 separate parts, I get no heat transfer across the interface. If I make the mesh from 2 bodies in a single part, OpenFOAM gives me an error related to the interface. It looks like "wall instead of mappedPatchBase". Does anyone know how to solve this?

[wyldckat]

Greetings Paul,

Originally Posted by Miner

This sounds a lot like a problem I have. I made a Fluent mesh and imported it using Fluent3DMeshToFoam. That worked fine. But I have a conjugate heat transfer problem, and if I make the fluid and solid meshes from 2 separate parts, I get no heat transfer across the interface. If I make the mesh from 2 bodies in a single part, OpenFOAM gives me an error related to the interface. It looks like "wall instead of mappedPatchBase". Does anyone know how to solve this?

Have you checked the solution given at http://www.cfd-online.com/Forums/ope...tml#post346373 post #9?

Best regards,
Bruno

[waiter120]

Hello, for everyone.
I want share my solution of converting ICEM CFD hex mesh to OpenFOAM mesh.
At start I have same problem as:

Cannot find metach for first face. cell model: tet first model face 3(1 2 3) mesh face:
4
(
...
...
)

The solution was found thanks to this amazing forum and all of its users.

So my recipe is like that.

1. Prepare mesh in ICEM CFD with all name selections
2. Export it to FLUENT_V6 (for my present experience, you don’t need specify BC in Output -> Boundary Condition (If I am wrong, please correct me))
3. Read mesh in FLUENT
4. Modify names of BC
4a. If you case is multi region (like chtMultiregionFoam). In FLUENT change type of coupled wall. From Wall to Interior (+ add interior- prefix to its name)
5. Change write-type to ascii “file/ binary-files? no”
6. Write .cas file
7. In OpenFOAM work directory
7a. fluentMeshToFoam –wrireZones fluent.cas
7b. splitMeshRegions -cellZones -overwrite

That’s ALL )))