Problem with Mesh conversion Gambit msh Foam
I have a problem to convert .msh file (obtained by
Gambit) to foam file. In fact the execution of the command fluentMeshToFoam I obtained that the mesh created. when I chek, the file blockMeshDict doasn't exist. with an other .msh file I did not have this problem, but a FOAMFATAL ERROR... (problem in Istream.C file). I hope know if somone success this conversion, and how can I do that? thanks |
You will not get a blockMeshD
You will not get a blockMeshDict. A blockMeshDict is the input file for OpenFOAM's own block mesher.
The fluentMeshToFoam will have written the polyMesh files (points, faces, cells). Mattijs |
indeed the changes had place i
indeed the changes had place in points, faces, cells but with the command I have
--> FOAM FATAL ERROR : Cannot find mesh description file "constant/polyMesh/blockMeshDict" or "constant/polyMesh/meshDescription" or "constant/mesh/meshDescription" thank you |
With what command?
With what command?
|
Hi,
Sorry if this sounds s
Hi,
Sorry if this sounds stupid, but why are you running the fluent converter on what I understand is a gambit mesh? How about using gambitToFoam instead? N |
Easy Tiger,
Fluent files w
Easy Tiger,
Fluent files will have the .msh and .cas extensions and you convert them with fluentMeshToFoam. Gambit files have the .neu extension and you use the gambitToFoam converter. Hrv |
I have some results in Fluen
I have some results in Fluent. and I want to run the same problem in Foam to compare. To do that I want to transform my mesh file from fluent to Foam but unfortunately I do not succeeded that, even I follow the instructions in Foam manual
I convert this file (.msh) with: >fluentMeshToFoamroot casename file.msh after that >blochMesh ... in the points, faces, cells files I have the informations but I can't view the mesh in paraview P.S. I'm new user of Foam |
>after that
>>blochMesh ...
>after that
>>blochMesh ... Why are you running blockMesh after fluentMeshToFoam? It makes no sense; blockMesh generates a mesh from a blockMeshDict mesh description file and has absolutely nothing to do with the mesh converters. |
ok
so how can I visualise m
ok
so how can I visualise my converted mesh thank you |
Use paraFoam
Use paraFoam
|
Here is my issue with a mesh o
Here is my issue with a mesh obtained by a third party from Gridgen, exported in Fluent .cas file (I was told that) and converted to polyMesh by fluentMeshToFoam:
No errors on outut from fluentMeshToFoam: dimension of grid: 3 Creating shapes for 3-D cells Creating patch for zone: 3 start: 1 end: 189360 type: interior name: interior-3 Patch 3 contains solid or internal faces. Not added to boundary Creating patch for zone: 4 start: 189361 end: 190440 type: wall name: side1-4 Creating patch for zone: 5 start: 190441 end: 192240 type: wall name: side3-5 Creating patch for zone: 6 start: 192241 end: 194400 type: inlet-vent name: inlet-vent-6 Creating patch for zone: 7 start: 194401 end: 196560 type: pressure-outlet name: pressure-outlet-7 Creating patch for zone: 8 start: 196561 end: 198360 type: wall name: side4-8 Creating patch for zone: 9 start: 198361 end: 199440 type: wall name: side2-9 Default patch type set to empty Checking mesh Writing mesh End ================================================ Then I made a LES case similar to channel395 and run it. The following error occurs : Create database Create mesh for time = 0 --> FOAM FATAL ERROR : face 0 and 540 areas do not match by 187.749% -- possible face ordering problem Function: cyclicFvPatch::makeWeights(scalarField& w) const in file: meshes/fvMesh/fvPatches/derivedFvPatches/cyclicFvPatch/cyclicFvPatch.Cat line: 62. FOAM aborting. I apreaciate if someone can help. Could email the original .cas mesh file if let me know how to do so. Thanks, Boyko |
Your cyclic faces are out of o
Your cyclic faces are out of order - this is not picked up from the fluent file.
Mattijs has written a tool which automatically reorders cyclic patches - he'll probably be able to give you more detail... Enjoy, Hrv |
It is called couplePatches. It
It is called couplePatches. It does not need a dictionary and you can run it with just the root and case. It should either tell you that the 'coupled patch face ordering ok' or something about morphing the mesh and will write the new mesh to a new time directory.
Just move that polyMesh/ directory back to constant/ (and check by running couplePatches again that the faces are now correctly ordered) Mattijs |
Hello,
I am trying to use a
Hello,
I am trying to use a pipe line mesh (theadres) created from fluent. It is a .msh extension mesh file. The converter fluenttofoam works apparently ok (when I use checkMesh, nothing wrong is noticed). However I have a problem with the cyclic condition: When I run icoFoam on my case I have the following error: ------------------------ -> FOAM FATAL ERROR : face 0 and 216 areas do not match by 3.49993% -- possible face ordering problem From function cyclicFvPatch::makeWeights(scalarField& w) const in file fvMesh/fvPatches/derivedFvPatches/cyclicFvPatch/cyclicFvPatch.C at line 58. ---------- So, after having consulted the forum I applied the command couplePatches to my case BUT it doen't create any new correct time polymesh directory. I have the following message from couplePatches: ----------------------------- Create time Create polyMesh for time = 0 Using geometry to calculate face correspondence across coupled boundaries (processor, cyclic) This will only work for cyclics if they are parallel or their rotation is defined across the origin Mesh has coupled patches ... Doing dummy mesh morph to correct face ordering ... --> FOAM Serious Error : From function cyclicPolyPatch::geometricOrder in file meshes/polyMesh/polyPatches/derivedPolyPatches/cyclicPolyPatch/cyclicPolyPatch.C at line 541 patch:inlet : Patch inlet gets decomposed in two zones ofinequal size: 432 and 0 This means that the patch is either not two separate regions or one region where the angle between the different regions is not sufficiently sharp. Please use topological matching or adapt the featureCos() setting Continuing with incorrect face ordering from now on! --> FOAM Serious Error : From function cyclicPolyPatch::geometricOrder in file meshes/polyMesh/polyPatches/derivedPolyPatches/cyclicPolyPatch/cyclicPolyPatch.C at line 541 patch:outlet : Patch outlet gets decomposed in two zones ofinequal size: 432 and 0 This means that the patch is either not two separate regions or one region where the angle between the different regions is not sufficiently sharp. Please use topological matching or adapt the featureCos() setting Continuing with incorrect face ordering from now on! Mesh ordering ok. Nothing changed. End ------------------------------------- Thanks if someone can help me, Anne |
Yes, I got the same message. H
Yes, I got the same message. How could I fix it?
/*---------------------------------------------------------------------------*\ | ========= | | | \ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \ / O peration | Version: 1.4.1 | | \ / A nd | Web: http://www.openfoam.org | | \/ M anipulation | | \*---------------------------------------------------------------------------*/ Exec : couplePatches . cylinder Date : Feb 12 2008 Time : 03:38:18 Host : daniel-desktop PID : 12053 Root : /home/daniel/OpenFOAM/daniel-1.4.1/run/tutorials/icoFoam Case : cylinder Nprocs : 1 Create time Create polyMesh for time = 0 Using geometry to calculate face correspondence across coupled boundaries (processor, cyclic) This will only work for cyclics if they are parallel or their rotation is defined across the origin Mesh has coupled patches ... Doing dummy mesh morph to correct face ordering ... cyclicPolyPatch::order : Number of faces per zonehttp://www.cfd-online.com/OpenFOAM_D...lipart/sad.gif71 71) --> FOAM Serious Error : From function cyclicPolyPatch::order(const primitivePatch&, labelList&, labelList&) const in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at line 726 patch:walls : Cannot match vectors to faces on both sides of patch half0Ctrs[0]http://www.cfd-online.com/OpenFOAM_D...lipart/sad.gif12.733 -15.2763 5) half1Ctrs[0]http://www.cfd-online.com/OpenFOAM_D...lipart/sad.gif0.407746 0.272448 5) Please use topological matching or adapt the featureCos() setting Continuing with incorrect face ordering from now on! Mesh ordering ok. Nothing changed. End |
I've got it working now.
Fo
I've got it working now.
For i made a mistake in my *.geo file like this, // Walls Physical Surface("walls wall") = {98,186,216,296,516,494,480,450,146,344,370,388,40 6,252,234,172}; and now I modified it to: // cylinder Physical Surface("cylinder wall") = {146,344,370,388,406,252,234,172}; // Walls Physical Surface("walls cyclic") = {98,186,216,296,516,494,480,450}; It works! |
i'm also geeting this message.
i'm also geeting this message. Can anyone help please
/*---------------------------------------------------------------------------*\ | ========= | | | \ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \ / O peration | Version: 1.4.1 | | \ / A nd | Web: http://www.openfoam.org | | \/ M anipulation | | \*---------------------------------------------------------------------------*/ Exec : couplePatches /home/admin/intern/project cyclic_igv_case Date : May 28 2008 Time : 10:00:49 Host : BGR-SW-99GML02 PID : 8679 Root : /home/admin/intern/project Case : cyclic_igv_case Nprocs : 1 Create time Create polyMesh for time = 0 Using geometry to calculate face correspondence across coupled boundaries (processor, cyclic) This will only work for cyclics if they are parallel or their rotation is defined across the origin Mesh has coupled patches ... Doing dummy mesh morph to correct face ordering ... cyclicPolyPatch::order : Number of faces per zonehttp://www.cfd-online.com/OpenFOAM_D...lipart/sad.gif15174 0) cyclicPolyPatch::order : Writing half0 faces to OBJ file "wall1_periodic_half0_faces.obj" cyclicPolyPatch::order : Writing half1 faces to OBJ file "wall1_periodic_half1_faces.obj" cyclicPolyPatch::order : Writing half0 face centres to OBJ file "wall1_periodic_half0.obj" cyclicPolyPatch::order : Writing half1 face centres to OBJ file "wall1_periodic_half1.obj" --> FOAM Serious Error : From function cyclicPolyPatch::order(const primitivePatch&, labelList&, labelList&) const in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at line 596 patch:wall1_periodic : Patch wall1_periodic gets decomposed in two zones ofinequal size: 15174 and 0 This means that the patch is either not two separate regions or one region where the angle between the different regions is not sufficiently sharp. Please use topological matching or adapt the featureCos() setting Continuing with incorrect face ordering from now on! cyclicPolyPatch::order : Number of faces per zonehttp://www.cfd-online.com/OpenFOAM_D...lipart/sad.gif15158 0) cyclicPolyPatch::order : Writing half0 faces to OBJ file "wall2_periodic_half0_faces.obj" cyclicPolyPatch::order : Writing half1 faces to OBJ file "wall2_periodic_half1_faces.obj" cyclicPolyPatch::order : Writing half0 face centres to OBJ file "wall2_periodic_half0.obj" cyclicPolyPatch::order : Writing half1 face centres to OBJ file "wall2_periodic_half1.obj" --> FOAM Serious Error : From function cyclicPolyPatch::order(const primitivePatch&, labelList&, labelList&) const in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at line 596 patch:wall2_periodic : Patch wall2_periodic gets decomposed in two zones ofinequal size: 15158 and 0 This means that the patch is either not two separate regions or one region where the angle between the different regions is not sufficiently sharp. Please use topological matching or adapt the featureCos() setting Continuing with incorrect face ordering from now on! Mesh ordering ok. Nothing changed. End Thanx in advance |
I am wondering if the couplePa
I am wondering if the couplePatches command is included in the OF 1.5. I received the message "command not found" when I typed in couplePatches
|
couplePatches has been integra
couplePatches has been integrated into createPatch, I think. Check release notes and/or User Guide, if I remember correctly there was some information about this issue.
Regards, Kati |
Thanks Kati,
I checked the
Thanks Kati,
I checked the release note and found out about the integration, although the User guide still listed couplePatches as a separate function. I will look around the forum and see if I can get the createPatch to work correctly. Thanks John |
All times are GMT -4. The time now is 22:18. |