|
[Sponsors] |
April 14, 2005, 14:55 |
Import gmsh msh to Foam
|
#1 |
Member
Ervin Adorean
Join Date: Mar 2009
Posts: 76
Rep Power: 17 |
Hi all,
I've finished a lovely 3D 1/8 engine mesh in gmsh, with hexahedral elements, saved it as version 1 .msh file and tried to apply gmshToFoam to it. I've exported the mesh 2 ways: 1. without physicals The error message I get is the following: Exec : gmshToFoam /home/ervin/OpenFOAM/ervin-1.1/run/tutorials/dieselEngineFoam motor2 motor2.msh Date : Apr 14 2005 Time : 19:12:05 Host : isi014.mot.upv.es PID : 18272 Root : /home/ervin/OpenFOAM/ervin-1.1/run/tutorials/dieselEngineFoam Case : motor2 Nprocs : 1 Create time Read nVerts:30615 Read nElems:38235 Mapping region 1000033 to Foam patch 0 Mapping region 1000035 to Foam patch 1 Mapping region 1000037 to Foam patch 2 Mapping region 1000039 to Foam patch 3 Mapping region 1000041 to Foam patch 4 Mapping region 1000043 to Foam patch 5 Mapping region 1000045 to Foam patch 6 Mapping region 1000047 to Foam patch 7 Mapping region 1000057 to Foam patch 8 Mapping region 1000059 to Foam patch 9 Mapping region 1000061 to Foam patch 10 Mapping region 2000069 to Foam patch 11 Mapping region 2000073 to Foam patch 12 Mapping region 2000076 to Foam patch 13 Mapping region 2000078 to Foam patch 14 Mapping region 2000087 to Foam patch 15 Mapping region 2000091 to Foam patch 16 Mapping region 2000095 to Foam patch 17 Mapping region 2000100 to Foam patch 18 Mapping region 2000109 to Foam patch 19 Mapping region 2000113 to Foam patch 20 Mapping region 2000117 to Foam patch 21 Mapping region 2000122 to Foam patch 22 Mapping region 2000134 to Foam patch 23 Mapping region 2000138 to Foam patch 24 Mapping region 2000139 to Foam patch 25 Mapping region 2000156 to Foam patch 26 Mapping region 2000160 to Foam patch 27 Mapping region 2000161 to Foam patch 28 Mapping region 2000170 to Foam patch 29 Mapping region 2000174 to Foam patch 30 Mapping region 2000178 to Foam patch 31 Mapping region 2000195 to Foam patch 32 Mapping region 2000199 to Foam patch 33 Mapping region 2000200 to Foam patch 34 Mapping region 2000209 to Foam patch 35 Mapping region 2000213 to Foam patch 36 Mapping region 2000217 to Foam patch 37 Mapping region 2000230 to Foam patch 38 Mapping region 2000234 to Foam patch 39 Mapping region 2000239 to Foam patch 40 Mapping region 2000248 to Foam patch 41 Mapping region 2000252 to Foam patch 42 Mapping region 2000256 to Foam patch 43 Mapping region 2000269 to Foam patch 44 Mapping region 2000273 to Foam patch 45 Mapping region 2000278 to Foam patch 46 Cells: total:28474 hex :27600 prism:874 pyr :0 tet :0 Patches: Patch Size 0 20 1 6 2 60 3 18 4 40 5 12 6 140 7 42 8 500 9 150 10 250 11 460 12 575 13 460 14 500 15 138 16 575 17 138 18 150 19 230 20 575 21 230 22 250 23 460 24 23 25 20 26 138 27 23 28 6 29 460 30 69 31 60 32 69 33 138 34 18 35 460 36 46 37 40 38 138 39 46 40 12 41 460 42 161 43 140 44 138 45 161 46 42 --> FOAM Warning : polyMesh::polyMesh(... construct from shapes...) : Found 8426 undefined faces in mesh; adding to default patch. --> FOAM FATAL ERROR : Problem : cannot find face 4(0 11 130 129) in patch Function: findFace in file: gmshToFoam.C at line: 108. FOAM aborting and 2. with physicals - created 5 physical surfaces and 1 physical volume In this case the error message is the following: Exec : gmshToFoam /home/ervin/OpenFOAM/ervin-1.1/run/tutorials/dieselEngineFoam motor2 motor1.msh Date : Apr 14 2005 Time : 19:47:43 Host : isi014.mot.upv.es PID : 19392 Root : /home/ervin/OpenFOAM/ervin-1.1/run/tutorials/dieselEngineFoam Case : motor2 Nprocs : 1 Create time Read nVerts:30615 Read nElems:42146 Mapping region 2000062 to Foam patch 0 Mapping region 2000065 to Foam patch 1 Mapping region 2000283 to Foam patch 2 Mapping region 2000284 to Foam patch 3 Mapping region 2000285 to Foam patch 4 Mapping region 2000286 to Foam patch 5 Cells: total:28474 hex :27600 prism:874 pyr :0 tet :0 Patches: Patch Size 0 4952 1 4952 2 828 3 1238 4 575 5 1127 --> FOAM Warning : polyMesh::polyMesh(... construct from shapes...) : Found 8426 undefined faces in mesh; adding to default patch. --> FOAM FATAL ERROR : Problem : cannot find face 4(0 11 130 129) in patch Function: findFace in file: gmshToFoam.C at line: 108. FOAM aborting The error is the same in the 2 cases. Can anybody please help me with this? Or a hint of what might be wrong? I can send the .geo & the .msh file if needed to check. Gmsh is a really nice 3D structured mesher and it's worth being able to use these meshes in Foam. Thanks. Ervin |
|
April 14, 2005, 15:06 |
Hi Ervin,
usually the probl
|
#2 |
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
Hi Ervin,
usually the problem is that in the .msh file there are no physical boundaries or too many. The converter - reads all volume elements - reads all surface elements - creates a mesh from all the volume elements (with all outside faces in a single patch) - then tries to match the surface elements (vertex by vertex) to the outside faces of the mesh and set the patch to the physical type of the surface element. Seems that matching is going wrong - it cannot find the surface element (0 11 130 129) in the mesh. Don't mind having a look at it. Can you send both files? |
|
April 15, 2005, 04:00 |
Hi Mattijs,
Sure I can. Jus
|
#3 |
Member
Ervin Adorean
Join Date: Mar 2009
Posts: 76
Rep Power: 17 |
Hi Mattijs,
Sure I can. Just tell me how. Or, to which address. Ervin |
|
April 15, 2005, 07:16 |
m.janssens at opencfd.co.uk. L
|
#4 |
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
m.janssens at opencfd.co.uk. Leave out the .msh file if it is too big - I have gmsh.
|
|
April 15, 2005, 07:32 |
I have sent you both files
|
#5 |
Member
Ervin Adorean
Join Date: Mar 2009
Posts: 76
Rep Power: 17 |
I have sent you both files
Thanks Ervin |
|
April 22, 2005, 15:15 |
Hi Mattijs,
Well, when I fi
|
#6 |
Member
Ervin Adorean
Join Date: Mar 2009
Posts: 76
Rep Power: 17 |
Hi Mattijs,
Well, when I finally set up a case with the engine mesh you've helped me to import, running dieselEngineFoam, produces this error: Exec : dieselEngineFoam /home/ervin/OpenFOAM/ervin-1.1/run/tutorials/dieselEngineFoam motor1 Date : Apr 22 2005 Time : 19:58:23 Host : isi014.mot.upv.es PID : 8381 Root : /home/ervin/OpenFOAM/ervin-1.1/run/tutorials/dieselEngineFoam Case : motor1 Nprocs : 1 Create engine time Create mesh for time = -0.02 --> FOAM FATAL ERROR : face 0 and 889 areas do not match by 31.4626% -- possible face ordering problem Function: cyclicFvPatch::makeWeights(scalarField& w) const in file: meshes/fvMesh/fvPatches/derivedFvPatches/cyclicFvPatch/cyclicFvPatch.C at line: 62. FOAM aborting When I imported the mesh into Foam it didn't complain. Do you think it's still a mesh (face ordering) problem, or it's something else I'm doing wrong? In the GMSH manual I found this: "Please note that the list of nodes and elements in Gmsh s mesh files do not have to be dense or ordered (i.e., the node and element numbers do not have to be given in a consecutive or even an ordered way). A sample C++ program to transform the formats so that all lists are dense and ordered is available in the source distribution ( utils/misc/mshsort.cpp ). This program is also a good example on how to read and write files in the .msh format." So I used this 'mshsort.cpp' to generate an 'ordered' mesh file, but the error message is the same. If you can find time, could you please have a look at mshsort.cpp utility? I would do it myself but my lack of C++ knowledge prevents me to. Thanks! Ervin |
|
April 23, 2005, 05:21 |
Hi Ervin,
This is OpenFOAM
|
#7 |
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
Hi Ervin,
This is OpenFOAM wanting the faces of corresponding cyclic faces ordered correctly. Run couplePatches on your case to write a new mesh with reordered faces. |
|
April 25, 2005, 05:40 |
Hi,
Now the error message i
|
#8 |
Member
Ervin Adorean
Join Date: Mar 2009
Posts: 76
Rep Power: 17 |
Hi,
Now the error message is: Create morphMesh for time = -180 Mesh has coupled patches ... Testing for correct face ordering ... --> FOAM Serious Error : cyclicPolyPatch::order : patch:slicefront : Patch gets decomposed in 1 zones 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 : cyclicPolyPatch::order : patch:sliceback : Patch gets decomposed in 1 zones 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! Patch face ordering OK. Coupled patch face ordering ok. Nothing changed ... End I have changed the 'slicefront' and 'sliceback' patch type to cyclic in the 'boundary' file. I don't understand what's wrong. The 'slicefront' and 'sliceback' represents each one 1 region. Ervin |
|
April 25, 2005, 07:23 |
The cyclic is both regions in
|
#9 |
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
The cyclic is both regions in one patch. Have a look at the user guide (search for 'cyclic')
|
|
April 25, 2005, 08:44 |
Hi,
What is the syntax for
|
#10 |
Member
Ervin Adorean
Join Date: Mar 2009
Posts: 76
Rep Power: 17 |
Hi,
What is the syntax for defining these 2 regions in 1 cyclic patch? slicefront { type cyclic; nFaces 1778; startFace 114404; } sliceback { type cyclic; nFaces 1778; startFace 117062; } Ervin |
|
April 25, 2005, 09:01 |
Q1) What do you think the foll
|
#11 |
New Member
Chris Greenshields
Join Date: Mar 2009
Posts: 28
Rep Power: 17 |
Q1) What do you think the following means?:
slicefront { type cyclic; nFaces 1778; startFace 114404; } |
|
April 25, 2005, 10:59 |
slicefront=arbitrary name of p
|
#12 |
Member
Ervin Adorean
Join Date: Mar 2009
Posts: 76
Rep Power: 17 |
slicefront=arbitrary name of patch
cyclic=base patch type nFaces=1778 quad type mesh faces, startFace=the index into the face list of the first face in the patch So, is it correct? slice { type cyclic; nFaces 1778x2; startFace 114404; } E |
|
April 25, 2005, 11:04 |
What's the syntax of faceList?
|
#13 |
Member
Ervin Adorean
Join Date: Mar 2009
Posts: 76
Rep Power: 17 |
What's the syntax of faceList?
Or for my question? |
|
April 25, 2005, 11:08 |
What is the syntax for definin
|
#14 |
Member
Ervin Adorean
Join Date: Mar 2009
Posts: 76
Rep Power: 17 |
What is the syntax for defining these 2 regions in 1 cyclic patch?
slicefront { type cyclic; nFaces 1778; startFace 114404; } sliceback { type cyclic; nFaces 1778; startFace 117062; } Ervin It's a simple Q |
|
April 25, 2005, 11:19 |
isn't this working?
slice
|
#15 |
Member
Tommaso Lucchini
Join Date: Mar 2009
Posts: 87
Rep Power: 17 |
isn't this working?
slice { type cyclic; nFaces 1778x2; startFace 114404; } |
|
April 25, 2005, 11:32 |
Hi Tommaso,
No, it's not wo
|
#16 |
Member
Ervin Adorean
Join Date: Mar 2009
Posts: 76
Rep Power: 17 |
Hi Tommaso,
No, it's not working: 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 Create morphMesh for time = -180 Mesh has coupled patches ... Testing for correct face ordering ... cyclicPolyPatch::order : Found 80 on patch slice where the cos of the angle between two connected faces was less than 0.9 cyclicPolyPatch::order : Writing zone 0 face centres to OBJ file "slice_zone_0.obj" cyclicPolyPatch::order : Writing zone 1 face centres to OBJ file "slice_zone_1.obj" cyclicPolyPatch::order : Writing zone 2 face centres to OBJ file "slice_zone_2.obj" cyclicPolyPatch::order : Number of faces per zone:3(1778 880 898) --> FOAM Serious Error : cyclicPolyPatch::order : patch:slice : Patch gets decomposed in 3 zones 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! Patch face ordering OK. Coupled patch face ordering ok. Nothing changed ... End I'm a beginner with this so I need exact answers. The question is still the same: Q) How EXACTLY do I have to define the cyclic patch for the two above mentioned regions. The geometry is 1/8 3D sector. Ervin |
|
April 25, 2005, 12:35 |
Hi,
I've got it working.
T
|
#17 |
Member
Ervin Adorean
Join Date: Mar 2009
Posts: 76
Rep Power: 17 |
Hi,
I've got it working. Thanks. Ervin |
|
April 27, 2005, 04:50 |
Hi!
I am a new user and I hav
|
#18 |
New Member
Amalia Apalategui
Join Date: Mar 2009
Posts: 13
Rep Power: 17 |
Hi!
I am a new user and I have a very basic question. I am trying to convert a gmsh mesh into foam. The gmsh file looks like $NOD $ENDNOD $ELM $ENDELM when I enter the following command gmshToFoam root case file.msh I get the error message --> FOAM FATAL IO ERROR : Attempt to get back from bad stream file: t10.msh at line 1. Function: void Istream::getBack(token& t) in file: db/IOstreams/IOstreams/Istream.C at line: 48. Can you tell me what I am doing wrong? Thanks a lot Amalia |
|
April 27, 2005, 05:15 |
The '$NOD' should be followed
|
#19 |
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
The '$NOD' should be followed by a number which is the number of vertices (nodes) following. I have
$NOD 29341 .. (29341 lines of coordinates) $ENDNOD $ELM 32132 .. (32132 lines of element data) $ENDELM |
|
April 27, 2005, 05:25 |
Thanks Mattijs,
my file has
|
#20 |
New Member
Amalia Apalategui
Join Date: Mar 2009
Posts: 13
Rep Power: 17 |
Thanks Mattijs,
my file has the number of vertices and elements. The file was in a wrong directory. :-( Now I get this error message Read nVerts:445 Read nElems:879 Mapping region 100 to Foam patch 0 Cells: total:0 hex :0 prism:0 pyr :0 tet :0 Patches: Patch Size 0 798 --> FOAM FATAL ERROR : faces deallocated Function: const faceList& polyMesh::allFaces() const in file: meshes/polyMesh/polyMesh.C at line: 562. FOAM aborting Aborted It seems that the mesh information is not correct in the mshfile. But I can visualize this mesh with gmsh (and in fact this mesh is one of the tutorial) Thanks a lot Amalia |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[blockMesh] Errors during blockMesh meshing | Madeleine P. Vincent | OpenFOAM Meshing & Mesh Conversion | 51 | May 30, 2016 11:51 |
[snappyHexMesh] How to define to right point for locationInMesh | Mirage12 | OpenFOAM Meshing & Mesh Conversion | 7 | March 13, 2016 15:07 |
decomposePar is missing a library | whk1992 | OpenFOAM Pre-Processing | 8 | March 7, 2015 08:53 |
MSH Import | Vivek Vasudevan | FLUENT | 6 | March 30, 2007 11:53 |
MSH file import | Vivek Vasudevan | Main CFD Forum | 2 | March 19, 2007 20:03 |