|
[Sponsors] |
[Commercial meshers] Fluent msh and cyclic boundary |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
September 4, 2009, 04:35 |
|
#41 |
Member
Tomislav Sencic
Join Date: Mar 2009
Posts: 42
Rep Power: 17 |
I solved my problem by modifying featureCos in
/home/tom/OpenFOAM/OpenFOAM-1.4.1-dev/src/OpenFOAM/meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C from 0.9999 to 0.99999999 or so, which allowed me tu use meshes of 179.5 degree central angle. |
|
December 20, 2009, 08:30 |
|
#42 |
Member
Join Date: Sep 2009
Posts: 45
Rep Power: 17 |
This can be a silly question, but can anyone explain what is the meaning of featureCos()
and featureCos 0.9 ? Thank you |
|
May 6, 2010, 04:02 |
how to solve
|
#43 |
New Member
jan
Join Date: Oct 2009
Posts: 6
Rep Power: 17 |
I made a mesh in Gambit, coupled the 'in' and 'out' edges, saved them together as 'wall', ran fluentMeshToFoam, ran createPatch with "symmetry" as posted here before and afterwards changed the type of my 'in_out' edge in polymesh/boundary to 'cyclic'
I still get : face 0 area does not match neighbour 321 by 53.8581% -- possible face ordering problem. patch:InOut my area:0.304138 neighbour area:0.528308 matching tolerance:0.001 Mesh face:1541679 vertices:4((100 50 3.04138) (100 49.95 3.04138) (100 49.95 -3.04138) (100 50 -3.04138)) Neighbour face:1542000 vertices:4((100 2.71793 3.04138) (100 2.71793 -3.04138) (100 2.80478 -3.04138) (100 2.80478 3.04138)) Rerun with cyclic debug flag set for more information. From function cyclicPolyPatch::calcTransforms() in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at line 180. FOAM exiting Anyone else with the same problem ? Last edited by fluent145; May 14, 2010 at 12:13. |
|
June 8, 2010, 08:58 |
cyclic sollution
|
#44 |
New Member
jan
Join Date: Oct 2009
Posts: 6
Rep Power: 17 |
I found the answer to my problem. Actually, it is all written here in previous post, but it took me a while to get all the pieces right. So I'll summarize it again here. I'm using Gambit and fluentMeshToFoam for the mesh.
GAMBIT 1. Link the "in" and "out" edges. It's the chain kinda looking button on the bottom left in the "Mesh edge" folder, and select "periodic" as-well. After that, just continue meshing as usual. 2. before exporting the mesh, I define both "in" and "out" (separately) as "wall". OF 3. run fluentMeshToFoam 4. in xx/constant/polymesh, edit the "boundary" file and change the type of both "in" and "out" to "symmetryPlane" 5. make a "createPatchDict" file and save it in xx/system. Mine looks like this : FoamFile { version 2.0; format ascii; class dictionary; location "system"; object createPatchDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // matchTolerance 1E-7; pointSync true; patches ( { name InOut; dictionary { type symmetryPlane; } constructFrom patches; patches (In Out); } ); 6. Run "createPatch" 7. createPatch should give you a new directory (like 0.02 or something, depending on your timestep) which looks like the polymesh directory. Go to xx/0.02/polymesh and open the "boundary" file. As you can see in the createPatchDict file, my "in" and "out" have chaged to one "InOut" edge. You will see "InOut" in the new boundary file with the type "symmetryPlane". Change this to "cyclic" and copy the whole directory to xx/contant/polymesh. 8. also, don't forget to adapt all your initial settings (files in xx/0) to contain the patch "InOut" with the type "cyclic". Then I just run channelFoam and it works . Good luck everyone ! |
|
January 28, 2011, 19:14 |
featureCos 0.9
|
#45 |
New Member
Brian Fiedler
Join Date: Jul 2009
Location: Norman, Oklahoma USA
Posts: 5
Rep Power: 17 |
||
March 23, 2011, 07:00 |
createPatch problem
|
#46 |
Senior Member
stephane sanchi
Join Date: Mar 2009
Posts: 314
Rep Power: 18 |
Dear OF users,
When I use the createPatch command I get the following error message. I have generated the mesh with ICEMCFD HEXA. It seems that an answer is to reorder (or renumber) the mesh faces ! Can someone explain me in details how to do it inside ICEM ? Thanks a lot for helping me, Stephane. Create time Reading createPatchDict. Using relative tolerance 0.001 to match up faces and points Create polyMesh for time = 0 Adding new patch sides as patch 5 from { type cyclic; } Moving faces from patch SYM1 to patch 5 Moving faces from patch SYM2 to patch 5 Doing topology modification to order faces. cyclicPolyPatch:rder : Writing half0 faces to OBJ file "sides_half0_faces.obj" cyclicPolyPatch:rder : Writing half1 faces to OBJ file "sides_half1_faces.obj" cyclicPolyPatch:rder : Dumping currently found cyclic match as lines between corresponding face centres to file "/shared/sanchi/OpenFOAM/sanchi-1.7.x/essai_hexa_MRF/sides_faceCentres.obj" --> FOAM Serious Error : From function cyclicPolyPatch:rder(const primitivePatch&, labelList&, labelList&) const in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at line 1557 Patch:sides : Cannot match vectors to faces on both sides of patch Perhaps your faces do not match? The obj files written contain the current match. Continuing with incorrect face ordering from now on! Dumping sides half0 faces to "coupled_sides_half0.obj" Dumping sides half1 faces to "coupled_sides_half1.obj" Dumping cyclic match as lines between face centres to "coupled_sides_match.obj" Synchronising points. On coupled patch sides forcing uniform rotation of (0.309017 -0.951057 -7.45058e-06 0.951057 0.309017 -4.04268e-06 6.14717e-06 -5.83666e-06 1) On coupled patch sides forcing uniform rotation of 1((0.309017 -0.951057 -7.45058e-06 0.951057 0.309017 -4.04268e-06 6.14717e-06 -5.83666e-06 1)) Synchronising points. --> FOAM Warning : From function syncPoints(const polyMesh&, pointField&, const CombineOp&, const point&) in file createPatch.C at line 482 There are decomposed cyclics in this mesh with transformations. This is not supported. The result will be incorrect Points changed by average:0.192361 max:11.7557 --> FOAM FATAL ERROR: face 0 area does not match neighbour 882 by 143.445% -- possible face ordering problem. patch:sides my area:13.7706 neighbour area:2.26757 matching tolerance:0.001 Mesh face:35523 vertices:4((4.39478 2.38451 0) (4.02876 -3.8254 4.08159) (4.43163 -4.20789 -5.1802e-05) (4.88308 2.64947 0)) Neighbour face:36405 vertices:4((3.62586 -3.44284 -4.23835e-05) (4.02875 -3.82536 -4.70928e-05) (4.43163 -4.20789 -5.1802e-05) (4.02876 -3.8254 4.08159)) Rerun with cyclic debug flag set for more information. From function cyclicPolyPatch::calcTransforms() in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at line 167. FOAM exiting |
|
March 23, 2011, 07:16 |
|
#47 |
Senior Member
stephane sanchi
Join Date: Mar 2009
Posts: 314
Rep Power: 18 |
Dear users,
with the following creatPatchDict file it works. After I will check if the computation runs as well. ----------------------- matchTolerance 1E-3; pointSync true; patchInfo ( { // Name of new patch name sides; // Type of new patch dictionary { type cyclic; transform rotational; rotationAxis (0 0 1); rotationCentre (0 0 0); } constructFrom patches; patches (SYM1 SYM2); } ); ----------------------- Without the following 3 lines it does not work ! transform rotational; rotationAxis (0 0 1); rotationCentre (0 0 0); Best regads, Stephane |
|
February 1, 2012, 14:25 |
|
#48 | |
Member
Aqua
Join Date: Oct 2011
Posts: 96
Rep Power: 15 |
Quote:
My mesh is created in Openfoam, by blockMesh, then SnappyHexMesh. Could you please tell me how to renumber the mesh? Thank you so much! Aqua |
||
January 25, 2013, 04:28 |
|
#49 |
Member
ali jafari
Join Date: Sep 2012
Posts: 50
Rep Power: 14 |
hi everybody
i used fluent3dmeshtofoam , and i did these suggestions , but this error apeared : matchTolerance 1E-7; pointSync true; // Patches to create. patches ( { // Name of new patch name p1_1; // Type of new patch dictionary { type cyclic; } // How to construct: either from 'patches' or 'set' constructFrom patches; // If constructFrom = patches : names of patches. Wildcards allowed. patches ("p1 p1_shadow"); // If constructFrom = set : name of faceSet set f0; } ); --> FOAM FATAL IO ERROR: keyword pointSync is undefined in dictionary "/home/ali/OpenFOAM/ali-2.1.1/run/tutorials/2Gesikes/system/createPatchDict" file: /home/ali/OpenFOAM/ali-2.1.1/run/tutorials/2Gesikes/system/createPatchDict from line 16 to line 20. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 400. FOAM exiting whats happen ? |
|
November 29, 2024, 22:16 |
|
#50 | |
Member
Anurag
Join Date: Feb 2023
Posts: 80
Rep Power: 3 |
Quote:
Hi fluent145, I am facing a similar issue as you and have posted my query in OpenFOAM, running and solving titled Periodic BC Error just today. Can you please look at the problem and let me know what do you think. Thanks |
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Cyclic boundaries importing Gambit msh file and interFoam | chegdan | OpenFOAM Running, Solving & CFD | 16 | February 14, 2023 04:56 |
[snappyHexMesh] Solution Snappy Hex 2D Msh with Surface Layers and cyclic bc for symmetric geometry | flexi182 | OpenFOAM Meshing & Mesh Conversion | 0 | May 24, 2013 09:38 |