|
[Sponsors] |
February 14, 2014, 10:57 |
More errors
|
#41 |
New Member
Luis Miguel
Join Date: Apr 2013
Location: Colombia
Posts: 13
Rep Power: 13 |
Hello Elia...
I've checked what you suggested me, I switch the vertices order and blockMesh runs well but now I've got a problem when I run checkMesh, the error is even worst, check this out: Valid index labels are 0..387999 --> FOAM Serious Error : From function bool zone::checkDefinition(const label maxSize, const bool report) const in file meshes/polyMesh/zones/zone/zone.C at line 211 Zone internal contains invalid index label 388092 Valid index labels are 0..387999 --> FOAM Serious Error : From function bool zone::checkDefinition(const label maxSize, const bool report) const in file meshes/polyMesh/zones/zone/zone.C at line 211 Zone internal contains invalid index label 388093 Valid index labels are 0..387999 --> FOAM Serious Error : From function bool zone::checkDefinition(const label maxSize, const bool report) const in file meshes/polyMesh/zones/zone/zone.C at line 211 Zone internal contains invalid index label 388094 Valid index labels are 0..387999 --> FOAM Serious Error : From function bool zone::checkDefinition(const label maxSize, const bool report) const in file meshes/polyMesh/zones/zone/zone.C at line 211 Zone internal contains invalid index label 388095 Valid index labels are 0..387999 --> FOAM Serious Error : From function bool zone::checkDefinition(const label maxSize, const bool report) const in file meshes/polyMesh/zones/zone/zone.C at line 211 Zone internal contains invalid index label 388096 Valid index labels are 0..387999 --> FOAM Serious Error : From function bool zone::checkDefinition(const label maxSize, const bool report) const in file meshes/polyMesh/zones/zone/zone.C at line 211 Zone internal contains invalid index label 388097 Valid index labels are 0..387999 --> FOAM Serious Error : From function bool zone::checkDefinition(const label maxSize, const bool report) const in file meshes/polyMesh/zones/zone/zone.C at line 211 Zone internal contains invalid index label 388098 Valid index labels are 0..387999 --> FOAM Serious Error : --> FOAM FATAL ERROR: Too many errors From function messageStream:perator OSstream&() in file lnInclude/messageStream.C at line 200. FOAM aborting #0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::error::abort() in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 Foam::messageStream:perator Foam::OSstream&() in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #3 Foam::messageStream:perator()(char const*, char const*, int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #4 Foam::zone::checkDefinition(int, bool) const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #5 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/checkMesh" #6 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/checkMesh" #7 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" #8 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/checkMesh" Aborted (core dumped) this is my new blockMesh file vertices ( ( -8 0 0 ) //1 ( 6 0 0 ) //2 ( 17 0 0 ) //3 ( 32 0 0 ) //4 ( -8 0.3 0 ) //5 ( 12 0.3 0 ) //6 ( 14 0.3 0 ) //7 ( 32 0.3 0 ) //8 ( -8 0.5 0 ) //9 ( 12 0.5 0 ) //10 ( 14 0.5 0 ) //11 ( 32 0.5 0 ) //12 ( -8 0 1 ) //13 ( 6 0 1 ) //14 ( 17 0 1) //15 ( 32 0 1) //16 ( -8 0.3 1 ) //17 ( 12 0.3 1) //18 ( 14 0.3 1) //19 ( 32 0.3 1) //20 ( -8 0.5 1) //21 ( 12 0.5 1) //22 ( 14 0.5 1) //23 ( 32 0.5 1) //24 ); blocks ( hex (0 1 5 4 12 13 17 16) ( 1000 120 1 ) simpleGrading (1 1 1) //block0 hex (2 3 7 6 14 15 19 18) ( 900 120 1 ) simpleGrading (1 1 1) //block1 hex (4 5 9 8 16 17 21 20) ( 1000 80 1 ) simpleGrading (1 1 1) //block2 hex (5 6 10 9 17 18 22 21) ( 100 80 1 ) simpleGrading (1 1 1) //block3 hex (6 7 11 10 18 19 23 22) ( 900 80 1 ) simpleGrading (1 1 1) //block4 ); edges ( ); boundary ( inlet { type patch; faces ( (0 12 16 4) (4 16 20 8) ); } bottom { type wall; faces ( (0 1 13 12) (1 5 17 13) (5 6 18 17) (6 2 14 18) (2 3 15 14) ); } outlet { type patch; faces ( (3 15 19 7) (7 19 23 11) ); } atmosphere { type patch; faces ( (8 9 21 20) (9 10 22 21) (10 11 23 22) ); } frontBack { type empty; faces ( (0 4 5 1) (2 6 7 3) (4 8 9 5) (5 9 10 6) (6 10 11 7) (12 13 17 16) (14 15 19 18) (16 17 21 20) (17 18 22 21) (18 19 23 22) ); } ); mergePatchPairs ( ); Any ideas how to fix the problem? thank you so much for your help |
|
February 14, 2014, 13:29 |
|
#42 |
New Member
Elia Daniele
Join Date: Mar 2010
Location: Oldenburg
Posts: 21
Rep Power: 16 |
Hallo Luis,
I've run your case in OF2.1.1. Everything is fine for me. I've attached the log of both blockMesh and checkMesh. Are you sure that you have cleaned the polyMesh folder before running blockMesh and checkMesh? Delete alla the files in constant/polyMesh except the blockMeshDict one. Try to run both applications again and see what happens. I think you have some old Zone file that conflicts with the new mesh. Hope it helps. Regards, Elia |
|
February 17, 2014, 12:04 |
mesh error solved
|
#43 |
New Member
Luis Miguel
Join Date: Apr 2013
Location: Colombia
Posts: 13
Rep Power: 13 |
Hi Ellia...
Your advice worked well the error has gone, but when I'm running in parallel I get an error in the MULES, I've read this is because of a bad decomposition in the geometric domain but I'm not sure if this error is due to the way I've created my mesh taking into account that my checkMesh now runs well, check this error out: Foam::error:rintStack(Foam::Ostream&)Foam::error :rintStack(Foam::Ostream&) at ??:? [0] #1 Foam::sigFpe::sigHandler(int) at ??:? [1] #1 Foam::sigFpe::sigHandler(int) at ??:? [1] #2 at ??:? [0] #2 in "/lib/x86_64-linux-gnu/libc.so.6" [0] #3 void Foam::MULES::limiter<Foam::geometricOneField, Foam::zeroField, Foam::zeroField>(Foam::Field<double>&, Foam::geometricOneField const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::zeroField const&, Foam::zeroField const&, double, double, int) in "/lib/x86_64-linux-gnu/libc.so.6" [1] #3 void Foam::MULES::limiter<Foam::geometricOneField, Foam::zeroField, Foam::zeroField>(Foam::Field<double>&, Foam::geometricOneField const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::zeroField const&, Foam::zeroField const&, double, double, int) at ??:? [0] #4 void Foam::MULES::limit<Foam::geometricOneField, Foam::zeroField, Foam::zeroField>(Foam::geometricOneField const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>&, Foam::zeroField const&, Foam::zeroField const&, double, double, int, bool) at ??:? What do you think of that? now I'm running without use parallel run and the simulation stops in the second 3.16 without any error, I mean still runs but it's not making any computation at all. thanks for your help Best regards. |
|
February 18, 2014, 02:42 |
|
#44 |
New Member
Elia Daniele
Join Date: Mar 2010
Location: Oldenburg
Posts: 21
Rep Power: 16 |
Hi Luis,
I cannot help you further with that. Since I have no experience with MULES scheme, that I think has something to do with VOF problems, I suggest you to open a new thread somewhere under VOF section, or something similar, maybe someone could help you more! Regards, Elia |
|
November 1, 2015, 13:52 |
Problem with mergePatchPairs
|
#45 |
New Member
|
Dear foamers,
I am quite newbie in the whole openfoam thing and I cannot wrap my head around the mesh stitching. I am trying to create a mesh consisting of several blocks (please consult the attached image) As I need the number of cells in one of the directions to change, I dividied all to different blocks. However, when I try to merge adjacent patches, I got the following error: Code:
--> FOAM FATAL ERROR: Zero length edge detected. Probable projection error: slave patch probably does not project onto master. Please switch on enriched patch debug for more info From function void enrichedPatch::calcCutFaces() const in file slidingInterface/enrichedPatch/enrichedPatchCutFaces.C at line 263. FOAM aborting Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ======== | | | \ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \ / O peration | Version: 2.3.0 | | \ / A nd | Web: www.OpenFOAM.org | | \/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "constant/polyMesh"; object blockMeshDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // convertToMeters 1; vertices ( ( 0.0 0.0 0.0 ) //0 ( 1.0 0.0 0.0 ) //1 ( 1.0 1.0 0.0 ) //2 ( 0.0 1.0 0.0 ) //3 ( 0.25 0.25 0.1 ) //4 ( 0.75 0.25 0.1 ) //5 ( 0.75 0.75 0.1 ) //6 ( 0.25 0.75 0.1 ) //7 ( 0.25 0.25 0.1 ) //8 ( 0.75 0.25 0.1 ) //9 ( 0.75 0.75 0.1 ) //10 ( 0.25 0.75 0.1 ) //11 ( 0.5 0.5 0.2 ) //12 ( 0.0 0.0 0.4 ) //13 ( 1.0 0.0 0.4 ) //14 ( 1.0 1.0 0.4 ) //15 ( 0.0 1.0 0.4 ) //16 ( 0.25 0.25 0.4 ) //17 ( 0.75 0.25 0.4 ) //18 ( 0.75 0.75 0.4 ) //19 ( 0.25 0.75 0.4 ) //20 ( 0.25 0.25 0.4 ) //21 ( 0.75 0.25 0.4 ) //22 ( 0.75 0.75 0.4 ) //23 ( 0.25 0.75 0.4 ) //24 ( 0.5 0.5 0.4 ) //25 ( 0.0 0.0 0.8 ) //26 ( 1.0 0.0 0.8 ) //27 ( 1.0 1.0 0.8 ) //28 ( 0.0 1.0 0.8 ) //29 ( 0.25 0.25 0.8 ) //30 ( 0.75 0.25 0.8 ) //31 ( 0.75 0.75 0.8 ) //32 ( 0.25 0.75 0.8 ) //33 ( 0.25 0.25 0.8 ) //34 ( 0.75 0.25 0.8 ) //35 ( 0.75 0.75 0.8 ) //36 ( 0.25 0.75 0.8 ) //37 ( 0.5 0.5 0.8 ) //38 ( 0.0 0.0 1.2 ) //39 ( 1.0 0.0 1.2 ) //40 ( 1.0 1.0 1.2 ) //41 ( 0.0 1.0 1.2 ) //42 ( 0.25 0.25 1.2 ) //43 ( 0.75 0.25 1.2 ) //44 ( 0.75 0.75 1.2 ) //45 ( 0.25 0.75 1.2 ) //46 ( 0.25 0.25 1.2 ) //47 ( 0.75 0.25 1.2 ) //48 ( 0.75 0.75 1.2 ) //49 ( 0.25 0.75 1.2 ) //50 ( 0.5 0.5 1.2 ) //51 ); edges ( ); blocks ( hex ( 0 1 5 4 13 14 18 17 ) ( 2 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 1 2 6 5 14 15 19 18 ) ( 2 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 2 3 7 6 15 16 20 19 ) ( 2 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 3 0 4 7 16 13 17 20 ) ( 2 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 8 9 12 12 21 22 25 25 ) ( 1 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 9 10 12 12 22 23 25 25 ) ( 1 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 10 11 12 12 23 24 25 25 ) ( 1 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 11 8 12 12 24 21 25 25 ) ( 1 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 13 14 18 17 26 27 31 30 ) ( 2 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 14 15 19 18 27 28 32 31 ) ( 2 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 15 16 20 19 28 29 33 32 ) ( 2 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 16 13 17 20 29 26 30 33 ) ( 2 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 21 22 25 25 34 35 38 38 ) ( 1 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 22 23 25 25 35 36 38 38 ) ( 1 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 23 24 25 25 36 37 38 38 ) ( 1 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 24 21 25 25 37 34 38 38 ) ( 1 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 26 27 31 30 39 40 44 43 ) ( 2 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 27 28 32 31 40 41 45 44 ) ( 2 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 28 29 33 32 41 42 46 45 ) ( 2 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 29 26 30 33 42 39 43 46 ) ( 2 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 34 35 38 38 47 48 51 51 ) ( 1 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 35 36 38 38 48 49 51 51 ) ( 1 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 36 37 38 38 49 50 51 51 ) ( 1 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) hex ( 37 34 38 38 50 47 51 51 ) ( 1 1 5 ) simpleGrading ( 1.0 1.0 1.0 ) ); boundary ( slave1 { type patch; faces ( ( 4 5 18 17 ) ( 17 18 31 30 ) ( 30 31 44 43 ) ( 5 6 19 18 ) ( 18 19 32 31 ) ( 31 32 45 44 ) ( 6 7 20 19 ) ( 19 20 33 32 ) ( 32 33 46 45 ) ( 7 4 17 20 ) ( 20 17 30 33 ) ( 33 30 43 46 ) ); } master1 { type patch; faces ( ( 8 9 22 21 ) ( 21 22 35 34 ) ( 34 35 48 47 ) ( 9 10 23 22 ) ( 22 23 36 35 ) ( 35 36 49 48 ) ( 10 11 24 23 ) ( 23 24 37 36 ) ( 36 37 50 49 ) ( 11 8 21 24 ) ( 24 21 34 37 ) ( 37 34 47 50 ) ); } ); mergePatchPairs ( ( master1 slave1 ) ); // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Best regards, Martin Note: I am also attaching a minimal example of the problematic case. |
|
December 30, 2015, 07:44 |
Problem with mergePatchPairs
|
#46 |
New Member
|
Dear Foamers,
back here again. The solution to my problem might be divided to the following steps:
Resulting mesh then looks (top view) like this: betterTopViewV2.jpg However, the resulting mesh is of a pure quality which can be seen on this solution (corresponds to water flow on steel, ReL = 60, interFoam): betterTopView.jpg Note: In my case, a much better approach was to replace the necessity of using "prism-like" blocks by using curved edges (polyLine). |
|
March 9, 2016, 12:04 |
Problem with mergePatchPairs
|
#47 |
New Member
Adam
Join Date: Mar 2016
Posts: 1
Rep Power: 0 |
Dear Foamers,
I am new to openFoam i would to like seek advice regarding meshing..here is my blockMeshDict,snappyHexMesh blockMeshDict.txt snappyHexMeshDict.txt after run blockMesh command it shows this after run blockMesh.txt snappyHexMesh and paraFoam..paraview only shows my stl file but do not have domain.. i hope someone can help me |
|
March 26, 2016, 06:13 |
|
#48 |
New Member
|
Hello Gates,
Did you manage to solve your problem? If not, please could you paste the commands you use to create your mesh? And also the corresponding logs (at least something like "after run snappyHexMesh". Best wishes, Martin |
|
May 29, 2016, 05:25 |
blockMesh error
|
#49 |
New Member
Join Date: May 2016
Posts: 2
Rep Power: 0 |
Hello to everyone, I have a problem while I'm trying to create my blockMesh. I've checked my mesh several times, but i cannot find the error. It shows me the message:
--> FOAM FATAL ERROR: Inconsistent number of faces between block pair 3 and 4 From function blockMesh::calcMergeInfo() in file blockMesh/blockMeshMerge.C at line 217. FOAM exiting Could anyone help me? |
|
May 29, 2016, 07:28 |
|
#50 |
New Member
Marco Atzori
Join Date: Mar 2016
Posts: 22
Rep Power: 10 |
Hi!
I tried to use your blockMeshDict, but I obtain a "bad" warning before the error: Code:
Creating block mesh topology --> FOAM Warning : From function polyMesh::polyMesh(... construct from shapes...) in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 903 Found 3 undefined faces in mesh; adding to default patch. BTW, if I remember properly, the error in itself could be related with the fact that you cannot put a vertex on an edge: a face can match with another face only, i.e.: edges should be enterly in common between near cells. Hope that helps! |
|
May 29, 2016, 21:32 |
|
#51 |
Senior Member
Join Date: Aug 2013
Posts: 407
Rep Power: 16 |
Hi,
Your problem comes from the following blocks: Code:
hex (4 9 10 5 33 38 39 34) (3 5 1) simpleGrading (1 1 1) hex (3 8 9 4 32 37 38 33) (6 26 1) simpleGrading (1 1 1) In your case, in the first instance, edge connected by the vertices 4 & 9 has 3 divisions. In the second instance, edge connected by the vertices 4 & 9 has 6 divisions. This is not allowed by blockMesh. Hope this helps. Cheers, Antimony |
|
May 30, 2016, 10:51 |
|
#52 |
New Member
Join Date: May 2016
Posts: 2
Rep Power: 0 |
Thank you very much for your help. I guess that if i want to dense my mesh, i have to use edgeGrading command. Am i right???
Thank you again! |
|
Tags |
blockmeshdict block mesh |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
How to use PIMPLE properly? | floquation | OpenFOAM Running, Solving & CFD | 27 | August 12, 2024 10:15 |
Transient simulation not converging | skabilan | OpenFOAM Running, Solving & CFD | 14 | December 16, 2019 23:12 |
pimpleDyMFoam computation randomly stops | babapeti | OpenFOAM Running, Solving & CFD | 5 | January 24, 2018 05:28 |
Stuck in a Rut- interDyMFoam! | xoitx | OpenFOAM Running, Solving & CFD | 14 | March 25, 2016 07:09 |
How to write k and epsilon before the abnormal end | xiuying | OpenFOAM Running, Solving & CFD | 8 | August 27, 2013 15:33 |