[Claudio]

Hi there,

I'm working on a case where the grid is built using enGrid. It all seems fine, but when I run CheckMesh (OpenFOAM) it fails 4 checks, and writes the culprits to 4 different cellSets.
How do I display these in Paraview?

I tried copy the entire constant folder over, with the sets subfolder in it, but no luck.

Thanks for any help.

Claudio

Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           900745
    internal points:  900745
    faces:            9630792
    internal faces:   9630792
    cells:            4748020
    boundary patches: 0
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     0
    prisms:        269504
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    4478516
    polyhedra:     0

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
    Patch               Faces    Points   Surface topology                  

Checking geometry...
    Overall domain bounding box (-15 -10 -10) (25 10 10)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (0 0 0) OK.
 ***Open cells found, max cell openness: 1, number of open cells 21134
  <<Writing 21134 non closed cells to set nonClosedCells
  <<Writing 245 cells with high aspect ratio to set highAspectRatioCells
    Minumum face area = 1.27259977e-07. Maximum face area = 10.29648759.  Face area magnitudes OK.
    Min volume = 1.666666667e-300. Max volume = 9.232429517.  Total volume = 31465.12518.  Cell volumes OK.
    Mesh non-orthogonality Max: 179.7735569 average: 15.80337767
   *Number of severely non-orthogonal faces: 8959.
 ***Number of non-orthogonality errors: 20686.
  <<Writing 29645 non-orthogonal faces to set nonOrthoFaces
 ***Error in face pyramids: 21214 faces are incorrectly oriented.
  <<Writing 21198 faces with incorrect orientation to set wrongOrientedFaces
 ***Max skewness = 216.0434447, 549 highly skew faces detected which may impair the quality of the results
  <<Writing 549 skew faces to set skewFaces
    Coupled point location match (average 0) OK.

Failed 4 mesh checks.

End

[tomf]

Hi Claudio,

You can use the foamToVTK utility to make VTK files of any set:

foamToVTK -faceSet nonOrthoFaces -time 0

You can than open your case in ParaView and open the vtk files for each set. Just check the names of the set from the checkMesh log and run foamToVTK for each faceSet. Do not forget the -time 0 or otherwise it may overwrite your old VTK files.

Regards,
Tom

[Madi]

Hello,

i got a familiar Question too. I do the FoamToVTK but when i load it in paraview i can't see my wrong points. What I'm doing wron?

Thanks.

Madi

[tomf]

Please tell me exactly what you did. From your question in the current form I can not help you, accept guessing what went wrong.

2 hints/questions:

1. What was the exact command you gave when running foamToVTK?
2. Did you open the VTK files that where created in ParaView?

Regards,
Tom

[Madi]

Hello Tom,
thanks for your Answer.

The command was: foamToVTK -pointSet nonAlignedEdges
Then I opend paraview with my case. After that I opend the VTK file and press apply. Then I changed the colour of the VTK to see it better. But nothing appears.

[tomf]

Hi Madi,

For a pointSet I recommend to use the glyph filter on the pointset with spheres and then vary the radius until they are visible. Points are just very small, which makes it difficult to see them.

This nonAlignedEdges is typically a problem for 2D cases, and it can usually be corrected by using the

flattenMesh

utility.

Regards,
Tom

[Madi]

Hi Tom

it worked. Thank you

[Tanne25]

Hi Tom,

I have a new question: When I use topoSet it will creates me alos sets in the constat file. Is it possible to look at them in the same way as i look at the errors in checkMesh. I tried to covert in VTK but it didn't work Can you help me again please?

Thanks

[tomf]

Hi Christine,

Maybe I could, but I would need to know exactly what you have. So please show me the output of topoSet that you have.

Regards,
Tom

[us7]

Originally Posted by tomf

Hi Christine,

Maybe I could, but I would need to know exactly what you have. So please show me the output of topoSet that you have.

Regards,
Tom

Hello Tom,
Can you tell me the way to visualize topoSet in paraView so i could see how actual geometry of topoSet looks like in the main mesh?

Regards,
Umer

[tomf]

Hi,

I would need a bit more information on what you want to do exactly? What is the set that results, what is the output from topoSet?

Regards,
Tom

[us7]

Originally Posted by tomf

Hi,

I would need a bit more information on what you want to do exactly? What is the set that results, what is the output from topoSet?

Regards,
Tom

Hello Tom,
I have created square (blockMeshDisct) of 10m and then i have set sediments shape inside this square using topoSet e.g. boxToCell and cylinderToCell. Simulation works fine but i don't know how to show the mesh or shape of topoSet in paraView. It only shows square mesh what i have given in blockMeshDict. Is there any way to see topoSet mesh/cells/shape in paraView?

Umer

[tomf]

Hi,

I would suggest to use:

foamToVTK -cellSet <cellSetName> -latestTime

I just added the latestTime option to limit the output to only the latest timestep.

You can than visualize the VTK file that follows from this. I do not think there is another option.

Regards,
Tom

[us7]

Originally Posted by tomf

Hi,

I would suggest to use:

foamToVTK -cellSet <cellSetName> -latestTime

I just added the latestTime option to limit the output to only the latest timestep.

You can than visualize the VTK file that follows from this. I do not think there is another option.

Regards,
Tom

Thank you very much. Its working and now i can see mesh separately.

Thanks again .

umer

[matejfor]

Hi, just to add to the topic for future reference, when using OpenFOAM v1706 (http://openfoam.com) you may run:

>> checkMesh -writeAllFields

to get all quality parameters written down as volScalarFields, so you may easily view the not-so-good-cells using a Threshold filter when reading in the appropriate time directory from paraview.

[LeeRuns]

Originally Posted by matejfor

Hi, just to add to the topic for future reference, when using OpenFOAM v1706 (http://openfoam.com) you may run:

>> checkMesh -writeAllFields

to get all quality parameters written down as volScalarFields, so you may easily view the not-so-good-cells using a Threshold filter when reading in the appropriate time directory from paraview.

in openfoam 7 we can now execute checkMesh with the writeSets option.

 
checkMesh -writeSets <output file type>

so if you want to go to paraview (like most ppl) then do this to get the vtk output

 
checkMesh -writeSets vtk