|
[Sponsors] |
[blockMesh] Problems in creating a wedge type mesh |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
May 25, 2010, 04:43 |
Problems in creating a wedge type mesh
|
#1 |
New Member
Join Date: May 2010
Posts: 3
Rep Power: 16 |
Hello,
I'm a newbie with OpenFOAM. I'd like to create a wedge type quasi 2d mesh with blockMesh. Inside the tutorials I found a matching case: /tutorials/multiphase/interFoam/les/nozzleFlow2D . But even with the help of this sample case and the documentation of OpenFoam I don't progress with my Problem. :confused: My Code: blockMeshDict.m4: Code:/*--------------------------------*- C++0/p: ...0/U: ... object U; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //dimensions [0 1 -1 0 0 0 0]; internalField uniform (0 0 0); boundaryField { rotatingWall { type rotatingWallVelocity; origin (0 0 0); // origin of axis and the axis axis (1 0 0); // about which the wall will rotate omega 100; // 1/s } rotAxis1 { type empty; } wallShroudBottom { type fixedValue; value uniform (0 0 0); } wallShroudLateral { type fixedValue; value uniform (0 0 0); } front { type wedge; } back { type wedge; } } // ************************************************** *********************** // And here the error prompt I get when running blockMesh: nProcs : 1 SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Creating block mesh from "/home/cfxuser/OpenFOAM/cfxuser-1.6/run/projects/001_einfach/constant/polyMesh/blockMeshDict" Creating blockCorners Creating curved edges Creating blocks Creating patches Creating block mesh topology Default patch type set to empty #0 Foam::error: :tongue:rintStack(Foam::Ostream&) in "/home/cfxuser/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so" #1 Foam::sigFpe::sigFpeHandler(int) in "/home/cfxuser/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so" #2 __restore_rt at sigaction.c:0 #3 Foam::wedgePolyPatch::initTransforms() in "/home/cfxuser/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so" #4 Foam::wedgePolyPatch::wedgePolyPatch(Foam::word const&, int, int, int, Foam: :tongue:PolyBoundaryMesh const&) in "/home/cfxuser/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so" #5 Foam: :tongue:PolyPatch::addwordConstructorToTable<Foam::wedgePoly Patch>::New(Foam::word const&, int, int, int, Foam: :tongue:PolyBoundaryMesh const&) in "/home/cfxuser/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so" #6 Foam: :tongue:PolyPatch::New(Foam::word const&, Foam::word const&, int, int, int, Foam: :tongue:PolyBoundaryMesh const&) in "/home/cfxuser/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so" #7 Foam: :tongue:PolyMesh: :tongue:PolyMesh(Foam::IOobject const&, Foam::Xfer<Foam::Field<Foam::Vector<double> > > const&, Foam::List<Foam::cellShape> const&, Foam::List<Foam::List<Foam::face> > const&, Foam::List<Foam::word> const&, Foam::List<Foam::word> const&, Foam::word const&, Foam::word const&, Foam::List<Foam::word> const&, bool) in "/home/cfxuser/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so" #8 Foam::blockMesh::createTopology(Foam::IOdictionary &) in "/home/cfxuser/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64GccDPOpt/blockMesh" #9 Foam::blockMesh::blockMesh(Foam::IOdictionary&) in "/home/cfxuser/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64GccDPOpt/blockMesh" #10 main in "/home/cfxuser/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64GccDPOpt/blockMesh" #11 __libc_start_main in "/lib64/libc.so.6" #12 _start at /usr/src/packages/BUILD/glibc-2.9/csu/../sysdeps/x86_64/elf/start.S:116 floating point exception Please help me with my problem, thanks in advance. Yours Joscha |
|
June 10, 2010, 12:40 |
Wedge Geometry
|
#2 |
New Member
Alan Kastengren
Join Date: Mar 2009
Posts: 3
Rep Power: 17 |
I just had a similar problem. As mentioned in the user's guide, the wedge geometry must straddle a coordinate plane. It appears that your geometry has one face on a coordinate plane. I did the same thing, and had floating point errors until I corrected it. I hope this helps.
|
|
June 21, 2010, 08:10 |
|
#3 | |
New Member
Join Date: May 2010
Posts: 3
Rep Power: 16 |
Quote:
I corrected my blockmeshDict - file like you said. --> Problem solved |
||
March 19, 2011, 07:02 |
|
#4 |
New Member
Join Date: Sep 2010
Posts: 16
Rep Power: 17 |
Thank you, I had the same problem and after checking that I had a face in the xz plane I corrected that and it worked.
|
|
January 31, 2012, 03:13 |
|
#5 | |
New Member
Join Date: Jan 2012
Posts: 5
Rep Power: 14 |
Quote:
If I understand well, the first points define the coordinate planes, so I don't see how a geometry can have no face on a coordinate plane. Sorry if my question seems stupid but I really need your help. Here is my (very simple) code: vertices ( (0 0 0) //0 (2000 0 0) //1 (2000 17 0) //2 (0 17 0) //3 (0 0 500) //4 (2000 0 500) //5 ); blocks ( hex (0 1 2 3 4 5 5 4) (2000 1 500) simpleGrading (1 1 1) ); edges ( ); patches ( empty axis ( (4 5 5 4) ) wedge front ( (0 4 5 1) ) wedge back ( (2 5 4 3) ) patch inlet ( (2 1 5 5) ) patch outlet ( (0 1 2 3) (4 0 3 4) ) ); |
||
January 31, 2012, 05:56 |
|
#6 |
New Member
Join Date: Sep 2010
Posts: 16
Rep Power: 17 |
Your front wedge is on the x,z plane, all points have y = 0. Maybe you can solve that by displacing all points in the y direction, i.e. use y = 1 and y = 18 on the z = 0 edges. Or by using symmetrical points, i.e. points with y = -17 and with y = 17 for the z = 0 edges.
Check this mesh I made recently, It's for OpenFOAM 2.0 and has several blocks, but it is not really complicated. It's a small rocket nozzle. Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.0.1 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object blockMeshDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // convertToMeters 0.001; vertices ( //Axis Points (-58.59 0 0) //0 (-10.1752 0 0) //1 (4.4139 0 0) //2 (38.94 0 0) //3 //Nozzle Points (Front) (-58.59 39.6004478247 1.9816740616) //4 (-10.1752 19.9750052079 0.9995833854) //5 (4.4139 18.4381283072 0.9226754397) //6 (38.94 24.1198187885 1.2069969379) //7 //Nozzle Points (Back) (-58.59 39.6004478247 -1.9816740616) //8 (-10.1752 19.9750052079 -0.9995833854) //9 (4.4139 18.4381283072 -0.9226754397) //10 (38.94 24.1198187885 -1.2069969379) //11 ); blocks ( hex (0 1 1 0 4 5 9 8) (40 1 30) simpleGrading (0.33 1 0.05) hex (1 2 2 1 5 6 10 9) (20 1 30) simpleGrading (1 1 0.05) hex (2 3 3 2 6 7 11 10) (30 1 30) simpleGrading (3 1 0.05) ); edges ( arc 4 8 (-58.59 39.65 0) arc 5 9 (-10.1752 20 0) arc 6 10 (4.4139 18.4612 0) arc 7 11 (38.94 24.15 0) arc 5 6 (0 18.0773797131 0.9046229638) arc 9 10 (0 18.0773797131 -0.9046229638) ); boundary ( inlet { type patch; faces ( (0 0 4 8) ); } outlet { type patch; faces ( (3 3 11 7) ); } nozzle { type wall; faces ( (4 5 9 8) (5 6 10 9) (6 7 11 10) ); } sideFront { type wedge; faces ( (0 1 5 4) (1 2 6 5) (2 3 7 6) ); } sideBack { type wedge; faces ( (1 0 8 9) (2 1 9 10) (3 2 10 11) ); } axis { type empty; faces ( (0 0 1 1) (1 1 2 2) (2 2 3 3) ); } ); mergePatchPairs ( );
__________________
Terrassa Rocket Team Blog: http://terrassarocketteam.blogspot.com/ Last edited by TRT; February 13, 2012 at 05:49. Reason: Added the header to the blockMeshDict code. |
|
February 7, 2012, 08:55 |
|
#7 |
New Member
Join Date: Jan 2012
Posts: 5
Rep Power: 14 |
Thank you very much TRT!
I managed to create my geometry. However, I have another problem when I try to compile with simpleFoam. It is not the subject of the original post but maybe you can help me once more. Here is the massage: --> FOAM FATAL IO ERROR: keyword div((nuEff*dev(grad(U).T()))) is undefined in dictionary "/home/nhurel/BE/simulations_OpenFoam/2d_axisymetrique/jet_libre/test_sans_6_7/system/fvSchemes::divSchemes" file: /home/nhurel/BE/simulations_OpenFoam/2d_axisymetrique/jet_libre/test_sans_6_7/system/fvSchemes::divSchemes from line 32 to line 39. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 395. FOAM exiting And here is my fvSchemes file: FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; grad(p) Gauss linear; grad(U) Gauss linear; } divSchemes { default none; div(phi,U) Gauss upwind; div(phi,k) Gauss upwind; div(phi,epsilon) Gauss upwind; div(phi,R) Gauss upwind; div(R) Gauss linear; div(phi,nuTilda) Gauss upwind; div((nuEff*dev(T(grad(U))))) Gauss linear; } laplacianSchemes { default none; laplacian(nuEff,U) Gauss linear corrected; laplacian((1|A(U)),p) Gauss linear corrected; laplacian(DkEff,k) Gauss linear corrected; laplacian(DepsilonEff,epsilon) Gauss linear corrected; laplacian(DREff,R) Gauss linear corrected; laplacian(DnuTildaEff,nuTilda) Gauss linear corrected; } interpolationSchemes { default linear; interpolate(U) linear; } snGradSchemes { default corrected; } fluxRequired { default no; p ; } Thanks a lot once more! |
|
February 7, 2012, 09:43 |
|
#8 |
New Member
Join Date: Sep 2010
Posts: 16
Rep Power: 17 |
I am not sure, since I have never touched the schemes file. However your error is:
Code:
div((nuEff*dev(grad(U).T()))) undefined Code:
div((nuEff*dev(T(grad(U))))) Code:
divSchemes { [...] div((nuEff*dev(grad(U).T()))) Gauss linear; } I hope this helps!
__________________
Terrassa Rocket Team Blog: http://terrassarocketteam.blogspot.com/ |
|
February 10, 2012, 04:07 |
|
#9 |
New Member
Join Date: Jan 2012
Posts: 5
Rep Power: 14 |
Indeed it works!
Thank you very very much! |
|
February 13, 2012, 05:29 |
|
#10 |
New Member
Michael Stiehm
Join Date: Sep 2010
Posts: 13
Rep Power: 16 |
Hello everybody,
I just built the nozzle, which TRT posted bevore and I got the checkMesh error message: ***Number of edges not aligned with or perpendicular to non-empty directions I read some threads to this topic, but I think that the nozzle-mesh is quite correct. I use OpenFoam-1.6-ext, could this be the "failure". Thanks Michael |
|
February 13, 2012, 05:45 |
|
#11 |
New Member
Join Date: Sep 2010
Posts: 16
Rep Power: 17 |
Take into account that the nozzle I posted is for OpenFOAM 2.0. The boundary definitions have changed a lot, maybe there is the problem as you said. For exemple:
OpenFOAM 1.7.1: Code:
patches ( wall nozzle ( (4 5 9 8) (5 6 10 9) (6 7 11 10) ) [...] ); Code:
boundary ( nozzle { type wall; faces ( (4 5 9 8) (5 6 10 9) (6 7 11 10) ); } [...] );
__________________
Terrassa Rocket Team Blog: http://terrassarocketteam.blogspot.com/ |
|
February 13, 2012, 06:32 |
|
#12 |
New Member
Michael Stiehm
Join Date: Sep 2010
Posts: 13
Rep Power: 16 |
Thanks for your reply,
I adapted your blockMeshDict to my version, so everything regarded to the blockMeshDict is fine. For the first simulations, a simple pipeflow, I ignored the errors and run the case and this seems to work. Interesting is also the fact, that checkMesh collect every point as "not aligned with or perpendicular to non-empty directions". But with foamToVTK you can see no points in paraView! Do you get any error message with OF-2.0? Greetings Michael |
|
April 2, 2013, 04:28 |
|
#13 |
New Member
MadEyeMoody
Join Date: Apr 2013
Posts: 1
Rep Power: 0 |
hello,
I have recently started using Openfoam. I need to form a wedge mesh for Axis symmetric jet. M getting the following error: /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.1.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 2.1.1-221db2718bbb Exec : blockMesh Date : Mar 30 2013 Time : 11:43:26 Host : "ubuntu" PID : 5658 Case : /home/striker/Desktop/jet nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Disallowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Creating block mesh from "/home/striker/Desktop/jet/constant/polyMesh/blockMeshDict" Creating curved edges Creating topology blocks Creating topology patches Creating block mesh topology Check topology Basic statistics Number of internal faces : 1 Number of boundary faces : 10 Number of defined boundary faces : 10 Number of undefined boundary faces : 0 Checking patch -> block consistency Creating block offsets Creating merge list --> FOAM FATAL ERROR: Inconsistent number of faces between block pair 0 and 1 From function blockMesh::calcMergeInfo() in file blockMesh/blockMeshMerge.C at line 221. FOAM exiting My blockMeshDict file is: /*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.1.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object blockMeshDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // convertToMeters 0.01; vertices ( (0 -0.034899 0.99939) //vertex 0 (150 -0.034899 0.99939) //vertex 1 //(0 0 150) //(0 0 0) (150 0.034899 0.99939) //vertex 2 (0 0.034899 0.99939) //vertex 3 (0 -3.4899 99.939) //vertex 4 (150 -3.4899 99.939) //vertex 5 (150 3.4899 99.939) //vertex 6 (0 3.4899 99.939) //vertex 7 (0 0 0) //vertex 8 (150 0 0) //vertex 9 ); blocks ( hex (8 9 9 8 0 1 2 3) (1 2 50) simpleGrading (1 1 1) hex (0 1 2 3 4 5 6 7) (1 198 50) simpleGrading (1 1 1) ); edges ( arc 0 3 (0 0 1) arc 1 2 (150 0 1) arc 4 7 (0 0 100) arc 5 6 (150 0 100) ); boundary ( Wall2 { type wall; faces ((0 4 7 3) //The wall above the jet ); } Wedgeplanes { type patch; faces ((1 0 8 9) (5 4 0 1) (8 3 2 9) (3 7 6 2) ); } axis { type empty; faces ((9 8 8 9) ); } faroffWall { type patch; faces ((4 5 6 7) ); } inlet { type patch; faces ((8 0 3 8) ); } outlet { type patch; faces ((9 2 1 9) (2 6 5 1) ); } ); mergePatchPairs ( ); //************************************************** *********************** // Can someone please help in rectifying the error? Thanks in Advance! |
|
April 2, 2013, 05:49 |
|
#14 |
Senior Member
Join Date: Aug 2010
Location: Groningen, The Netherlands
Posts: 216
Rep Power: 19 |
Hey
--> FOAM FATAL ERROR: Inconsistent number of faces between block pair 0 and 1 means in one of the directions the number of cells is not the same as on the adjunct edge dependant on how the edges are oriented or that the grading is not consistent regards Last edited by colinB; April 3, 2013 at 10:28. Reason: (delete false information) |
|
June 2, 2013, 02:53 |
|
#15 |
Member
Join Date: Oct 2012
Posts: 47
Rep Power: 14 |
hi
i want to creat a c-meh in blockmesh please please can you help me? there is this error: Create time Creating block mesh from "/home/shirin/OpenFOAM/shirin-2.1.x/run/tutorials/mesh/snapp/block/constant/polyMesh/blockMeshDict" Creating curved edges Creating topology blocks Creating topology patches Check topology #0 Foam::error:rintStack(Foam::Ostream&) in "/opt/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64Gcc46DPOpt/lib/libOpenFOAM.so" #1 Foam::sigSegv::sigHandler(int) in "/opt/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64Gcc46DPOpt/lib/libOpenFOAM.so" #2 in "/lib64/libc.so.6" #3 Foam::blockMesh::checkBlockMesh(Foam:olyMesh const&) const in "/opt/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64Gcc46DPOpt/lib/libblockMesh.so" #4 Foam::blockMesh::createTopology(Foam::IOdictionary const&, Foam::word const&) in "/opt/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64Gcc46DPOpt/lib/libblockMesh.so" #5 Foam::blockMesh::blockMesh(Foam::IOdictionary const&, Foam::word const&) in "/opt/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64Gcc46DPOpt/lib/libblockMesh.so" #6 in "/opt/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64Gcc46DPOpt/bin/blockMesh" #7 __libc_start_main in "/lib64/libc.so.6" #8 at /home/abuild/rpmbuild/BUILD/glibc-2.14.1/csu/../sysdeps/x86_64/elf/start.S:116 Segmentation fault |
|
June 2, 2013, 04:27 |
|
#16 |
Member
Yosmcer Mocktai
Join Date: Apr 2013
Location: Behind a computer
Posts: 50
Rep Power: 17 |
Hello sh.d,
As I understand, the software has a problem to merge the face 3 10 8 1 between the wedge and the hex (and for the other wedge, 3 10 12 5) because there are a face in 1 8 8 1. So a solution could be to put the 0 faces at the nose of your mesh, so in 0 7 7 0. I tried this and it works*: Code:
hex (0 3 1 0 7 10 8 7) (6 4 1) simpleGrading (1 1 1) hex (3 4 2 1 10 11 9 8) (6 4 1) simpleGrading (1 1 1) hex (0 5 3 0 7 12 10 7) (6 4 1) simpleGrading (1 1 1) hex (5 6 4 3 12 13 11 10) (6 4 1) simpleGrading (1 1 1) *I just tested the blocks, I deleted all the boundary definition and the curved edges for my try. So it might be errors theres. I checked the blocks with 'paraFoam -block". Be careful for your face definition in the boundary section: (0 1 7 8) is not correct, (0 7 8 1) is better; (13 4 11 6) is incorrect, (13 6 4 11) is better. (7 10 8) should be (7 10 8 7), same for the other 'triangular" faces (note that I use the new block definition I suggested here). [EDIT] after corrected the patches error, I get this mesh (attached, and blockMeshDict used too). |
|
June 2, 2013, 09:59 |
|
#17 |
Member
Join Date: Oct 2012
Posts: 47
Rep Power: 14 |
thank you very very much
|
|
July 28, 2013, 13:22 |
|
#18 |
Member
david
Join Date: Jun 2013
Location: Montreal, Canada
Posts: 62
Rep Power: 12 |
Good Day ...
__________________
Million Thanks, David "Small Dream is a Crime" |
|
January 10, 2014, 15:59 |
importance of starting vertex index in boundary patch
|
#19 |
New Member
Join Date: May 2013
Posts: 6
Rep Power: 13 |
I have created a blockMeshDict file to generate a 2D cylindrical wedge, split in 4 parts, so that I can apply different grading. I am currently working in OpenFoam 2.2.1. You can find the file below. The blockMesh utility was giving me an error message:
Code:
face 0 in patch 1 does not have neighbour cell face: 4(0 3 9 0) As I spent a lot of time trying to figure out this "bug", I wanted to share this with you. Code:
FoamFile { version 2.0; format ascii; class dictionary; object blockMeshDict; } convertToMeters 0.001; vertices ( (0 0 0) (50 0 0) (100 0 0) (0 49.9524 2.18097) (50 49.9524 2.18097) (100 49.9524 2.18097) (0 99.9048 4.36194) (50 99.9048 4.36194) (100 99.9048 4.36194) (0 49.9524 -2.18097) (50 49.9524 -2.18097) (100 49.9524 -2.18097) (0 99.9048 -4.36194) (50 99.9048 -4.36194) (100 99.9048 -4.36194) ); blocks ( hex (0 1 10 9 0 1 4 3 ) (15 15 1) simpleGrading (1 1 1) hex (9 10 13 12 3 4 7 6 ) (15 15 1) simpleGrading (1 1 1) hex (1 2 11 10 1 2 5 4 ) (15 15 1) simpleGrading (1 1 1) hex (10 11 14 13 4 5 8 7 ) (15 15 1) simpleGrading (1 1 1) ); edges ( arc 6 12 (0 100 0) arc 7 13 (50 100 0) arc 8 14 (100 100 0) ); boundary ( axis { type empty; faces ( (0 1 1 0) (1 2 2 1) ); } inlet { type patch; faces ( (3 9 0 0) (3 6 12 9) ); } outlet { type patch; faces ( (2 11 5 2) (8 5 11 14) ); } front { type wedge; faces ( (0 1 4 3) (1 2 5 4) (3 4 7 6) (4 5 8 7) ); } back { type wedge; faces ( (0 9 10 1) (1 10 11 2) (9 12 13 10) (10 13 14 11) ); } walls { type wall; faces ( (6 7 13 12) (7 8 14 13) ); } ); mergePatchPairs ( ); |
|
February 15, 2015, 10:35 |
Wedge trouble
|
#20 |
Member
Gareth
Join Date: Jun 2010
Posts: 56
Rep Power: 16 |
Hi can anyone tell me what i am defining wrong in my blockMesh?
I followed this thread for the way to make a wedge using the hex definition in openFoam but i am still getting an error... Creating curved edges Creating topology blocks Creating topology patches Creating block mesh topology --> FOAM FATAL ERROR: face 2 in patch 1 does not have neighbour cell face: 4(7 8 17 16) Please find my BlockMeshDict attached.. any help would be appreciated. |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[blockMesh] 3-D Mesh in a cylinder | Nikunj.R | OpenFOAM Meshing & Mesh Conversion | 32 | July 9, 2023 13:22 |
[Commercial meshers] Problems with ANSYS mesh conversion | tdog | OpenFOAM Meshing & Mesh Conversion | 1 | March 31, 2016 17:36 |
[mesh manipulation] Importing Multiple Meshes | thomasnwalshiii | OpenFOAM Meshing & Mesh Conversion | 18 | December 19, 2015 18:57 |
Problem with geometry - concentric cylinders | Rhoddwen | OpenFOAM Running, Solving & CFD | 0 | December 15, 2014 09:22 |
[Commercial meshers] Trimmed cell and embedded refinement mesh conversion issues | michele | OpenFOAM Meshing & Mesh Conversion | 2 | July 15, 2005 04:15 |