When I do mesh conversion (gmshToFoam), I can see some additional boundary patches are created named as defaultFaces. In constant/polymesh/boundary I can see
defaultFaces { type patch; nFaces 4682; startFace 41763839; }
It is a full phase 3D geometry What should I do that in the 0/U and 0/p file? Should I add these default faces as patch in 0 folder boundary condition files?
Hello Sudipta, the default faces are the faces that you didn't include in any boundary while creating the mesh in Gmsh. All the faces in your 3D domain have to included in any one of the boundaries of the 3D domain that you created in Gmsh. So, I think the issue can be treated from Gmsh, however, I have not tried using Gmsh.
Hi Sudipta,
I am facing the same problem in my work. despite I am doing what Avijit Karmakar is saying, but the problem is still there.
The solution that I am using is that after conversion, I open the mesh with paraFoam and see which patch is that one called defaultFaces and then I change its name in "constant/polyMesh/boundary" file. Of course in my case I have usually 4 faces, which are not so many.
Another soultion is to automate the name conversion using changeDict tool.
Hello Sudipta Saha
gmshToFoam commands add all boundary faces of mesh to "defaultFaces", then it allocates different faces from "deafultFaces" to corresponding patches as mentioned in the script. If at the end defaultFaces has no faces then it is removed automatically, else remaining patches are named as "defaultFaces".
Yes, you can add suitable boundary conditions for "defaultFaces", but before doing this, check the faces allocated to "defaultFaces".
I hope the above explanation will clear your doubt.
Hello
First of all, please check in ParaView and see if the "deafultFaces" boundary is an internal face or one of your normal boundaries.
If it refers to one of your normal boundaries, then simply rename it to inlet, wall, ...
otherwise, your mesh contains internal faces.
In this case, perhaps
https://www.cfd-online.com/Forums/openfoam-meshing/84063-remove-internal-patch-es.html
or
http://openfoamwiki.net/index.php/Howto_importing_fluent_mesh_with_internal_walls
could be useful
Khaled Yassin Thanks a lot for your comment.
1. So you replace the defaultFaces word with something else?
2. That should also be included in 0/U and 0/p file, right? The faces that I am dealing with are basically invisible to the flow. I mean the are 'faces' but do not represent any boundary condition in the fluid flow. Suppose I have one cylinder inside a cylinder-- and the only thing that matters is the wall of the small cylinder-a no slip boundary condition. But the to plane faces does not represent any boundary because fluid just go through them. (The inlet and outlet are the the plane faces of the bigger cylinder)
Hi Sudipta Saha,
1. Yes, just rename it if you don't want to do any change to what you already have.
2. If you are defining an "imaginary" cylinder that should have no effect on the flow, then you should define it as a faceZone and then use it to create baffles using createBaffles tool in OpenFOAM.
In brief, baffles are two back to back boundaries with cyclic boundary conditions which means that what gets through the first comes out from the second. So, the resultant will be nothing.
You can know more from this video:
https://www.google.com/url?sa=t&rct=j&q=&esrc=s&source=web&cd=&cad=rja&uact=8&ved=2ahUKEwjZ_vn6mvXqAhXE2aQKHXScChQQwqsBMAF6BAgMEAQ&url=https%3A%2F%2Fwww.youtube.com%2Fwatch%3Fv%3D7Ex1RHDQqIc&usg=AOvVaw3KLGFpiUlF8bVbfL7BfTJp
or from OpenFoam wiki page: https://openfoamwiki.net/index.php/CreateBaffles
You can fina a tutorial that is using this tool in : tutorials/multiphase/interPhaseChangeFoam/propeller/
- Badges
- Science topic