fluentMeshToFoam multidomain mesh conversion problem
Hi all,
I have an ICEM CFD mesh, I exported it to fluent .msh format, and now I want to covert it to OF format using fluentMeshToFoam. The mesh has 3 interfaces between Inlet-Rotor-Stator domains. The interface constists of 1 faces what belongs to both domains. Could it be the problem? Should I have two overlapping faces as interfaces? Thank you, Attila Quote:
|
Hi Attila,
you could try fluent3DMeshToFoam instead of fluentMeshToFoam. Philip |
Hi,
thanks, I already tried it. Seems to me that fluentMeshToFoam doesn't handle multidomain mesh. Now I can convert the mesh using fluent3DMeshToFoam. If I set the name of interface as "interface" OF recognizes and removes it so finally I have one domain. If I change the name of it to wall in ICEM, I'll have the wall inside the domain, but only one. I need 2 to use the AMI approach. Or am I wrong? What mesh manipulation utility can be used to double the interface and how? Thank you in advance! |
Attila,
I am not sure how to split one wall into two. I would export each region separately from ICEM to separate OpenFOAM cases and then merge them into one mesh (with two boundaries at the interface) using mergeMeshes. Philip |
Hi, thank you for your reply!
I made it on a testcase, but I'm getting errors. I exported the two separate meshes as Fluent format, converted using fluent3DmeshToFoam and typed: mergeMeshes OFsimulation OFsimulation2 executed from the root directory of these cases. Quote:
|
I've started over, and now I have the merged mesh, but in the directory belongs to the first time step. Do you know why? Should I copy the results to the constant/ploymesh directory?
Thank you very much! |
Quote:
Philip |
Thank you Philip, it should be OK now.
Have a nice day, Attila |
And indeed, the method is working perfectly. So for other who are interested:
1. Create the mesh in icem, using 1 face as interface 2. save every domain separately by deleting the other parts for instance. save with the interfaces, by rename it to AMI1 for example. The other domain will have AMI2 obviously 3. export the mesh using fluent V6 format 4. create separate case directories, put the .msh files there 5. run fluent3DMeshToFoam for every directories 6. run mergeMeshes masterDict Slavedict command as many times as much domains you have 7. modifiy the files in constant, system and 0 directory as usual (by using the propeller tutorial for instance) and it should work. Thanks again to Philip. |
Quote:
I have tried using chtMultiregionFoam for conjucate heat transfer. when you tranfoem the grid from fluent to openfoam and try SpiltRegions utility, it creates an interface between the two zones. on that interface , there is one boundary condition in Zone1 and another boundary Condition for Zone2. but imagine if i have a solid block in the flow stream which two of two of its faces are insulated and the remainging are conductive. in that case how can i define a boundary condition?!!! :confused: ( the interface between solid and liquid will be one patch). Best Mehdi |
I'm not experienced in it, sorry. Do you really need two patches on the fluid-solid interface? In this case it should be consistent, I mean same heat flux etc. If you want it insulated, you can use heat flux = 0 BC as well, but I really don't have experience with it in OpenFOAM.
Good luck |
Quote:
Hi Attesz I do the similar things with you , but I just delete the interface shell mesh and delete the interface surface. I do nothing with AMI, while Openfoam still can run and the velocity is satisfactory... why is this happen? |
Hello, for everyone. I want share my solution of converting ICEM CFD hex mesh to OpenFOAM mesh.
This 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 ))) |
All times are GMT -4. The time now is 17:54. |