[luigi21]

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

[fakekarma]

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

[luigi21]

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.

[fakekarma]

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

[Ramwi]

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:

--> 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

my blockMeshDict is:

/*--------------------------------*- 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    ) 
); 

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Please, I would be gratefull for any advice.

Best regards,
Martin

Note: I am also attaching a minimal example of the problematic case.

[Ramwi]

Dear Foamers,

back here again. The solution to my problem might be divided to the following steps:

1. Divide the mesh to completely separate blocks (I divided it to 4 prisms which did not share any vertices).
2. Subdivide the resulting prisms by the "layers" which should contain different number of cells
3. Merge resulting patches in 1 direction by mergePatchPairs
4. Merge the rest of the patches using stitchMesh utility
5. Use zipUpMesh utility to improve the mesh quality

Note: Also, it is much better to use higher number of cells.


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).

[Gates]

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

[Ramwi]

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

[thanasisB]

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?

[Atzori]

Hi!
I tried to use your blockMeshDict, but I obtain a "bad" warning before the error:

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.

I advise you to solve this warning before: check again the faces (I know: it is very boring).
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!

[Antimony]

Hi,

Your problem comes from the following blocks:

 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)

And is related to the fact that unless you have duplicate vertices defining duplicate lines, you cannot have different mesh resolutions on an edge.

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

[thanasisB]

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!