[cfdopenfoam]

dear foamers.

i am now confused by the -1 pointIndex in paraView, as what has been attached. although the polyMesh is generated manually, i firstly do not think this comes from the files in polyMesh folder because it seems that the geometry and topology can be recognized. besides, the pointIndex -1 seems to correspond to the cell type (Pyramid and Tetrahedron).

i am very sorry that my mesh files could not be uploaded correctly. could someone give some hints or suggestions with the attached image?
thanks a lot!

/karelke

[wyldckat]

Quick question: How exactly are you getting these arrays named "Point Index *"? Did you use a filter in ParaView to generate these fields?
Because my guess is that these fields were loaded from the time folder, e.g. from the folder "0".

[cfdopenfoam]

Originally Posted by wyldckat

Quick question: How exactly are you getting these arrays named "Point Index *"? Did you use a filter in ParaView to generate these fields?
Because my guess is that these fields were loaded from the time folder, e.g. from the folder "0".

thanks very much for your reply, Bruno.

i am working on paraview 4.1.0 and i think i do not use any filter to generate fields. i just want to view the mesh and paraview gives me this strange results. i choose the Spreadsheet View option and change the Attribute from fields to cell data because i just intend to view the mesh. and then i got what shown in the attached image.

checkMesh gives:

Checking geometry...
    Overall domain bounding box (1.12393e+06 -1.69078e+06 -0.5) (1.25165e+06 -1.54424e+06 0.5)
    Mesh (non-empty, non-wedge) directions (1 1 0)
    Mesh (non-empty) directions (1 1 0)
    All edges aligned with or perpendicular to non-empty directions.
 ***Boundary openness (-0.0010534 -0.00041202 0) possible hole in boundary description.
 ***Open cells found, max cell openness: 1, number of open cells 2170
  <<Writing 2170 non closed cells to set nonClosedCells
 ***Zero or negative face area detected.  Minimum area: 0
  <<Writing 6 zero area faces to set zeroAreaFaces
 ***Zero or negative cell volume detected.  Minimum negative volume: -1.90841e+06, Number of negative volume cells: 2155
  <<Writing 2155 zero volume cells to set zeroVolumeCells
    Mesh non-orthogonality Max: 179.997 average: 161.432
   *Number of severely non-orthogonal (> 70 degrees) faces: 1.
 ***Number of non-orthogonality errors: 2131.
  <<Writing 2132 non-orthogonal faces to set nonOrthoFaces
 ***Error in face pyramids: 10760 faces are incorrectly oriented.
  <<Writing 8643 faces with incorrect orientation to set wrongOrientedFaces
 ***Max skewness = 3.28738e+302, 24 highly skew faces detected which may impair the quality of the results
  <<Writing 24 skew faces to set skewFaces
    Coupled point location match (average 0) OK.

Failed 8 mesh checks.

and the output files are attached. if the mesh files are needed, please let me know.

thanks very much!

[wyldckat]

Hi Karelke,

I can't do much with the files from the "sets" folder, because they only provide the lists of indexes and none of them are "-1". Therefore, if the mesh cannot be provided in public, please send me a DropBox link or similar via private message.

The output from checkMesh is a considerably great reason for concern, because even hard to believe that solver will not crash with such a mesh.
In addition, having the mesh located at such a large distance from the origin of the referential:

(1.12393e+06 -1.69078e+06 -0.5) (1.25165e+06 -1.54424e+06 0.5)

means that you have the mesh at around 150km away from the origin of the referential. This can potentially lead to some considerable calculation errors. You can use the utility transformPoints to move the mesh to a location closer to the origin:

transformPoints -translate '(-1.12393e+06  1.69078e+06 0.0)' -region networkMesh

By the way, how are you generating the mesh?

edit: I forgot to ask: What files do you have inside the folder "0/networkMesh"?

Best regards,
Bruno

[wyldckat]

Hi Karelke,

I've received the files with success. I'm unable to reproduce the same issue you're getting.
I need to know more details, namely:

1. Which OpenFOAM version are you using?
2. Which ParaView version are you using?
3. Which options did you use to load the file you opened in ParaView? I'm referring to the ones in the widget (part of the window) named "Properties", where we configure what fields to load and with what settings, as shown in the attachment below.

Best regards,
Bruno

[cfdopenfoam]

Originally Posted by wyldckat

Hi Karelke,

I've received the files with success. I'm unable to reproduce the same issue you're getting.
I need to know more details, namely:

1. Which OpenFOAM version are you using?
2. Which ParaView version are you using?
3. Which options did you use to load the file you opened in ParaView? I'm referring to the ones in the widget (part of the window) named "Properties", where we configure what fields to load and with what settings, as shown in the attachment below.

Best regards,
Bruno

thanks, Bruno.

1. OF 2.3.0
2. paraview 4.1.0 (no problem detected for other simple cases)
3. i did the same with you.

what if you check the mesh with checkMesh?

what if you choose the spreadsheet view as shown in the attached image.
after that, you can change the Attribute entry from point data to cell data, and sort the sheet by cell type. (see attached image)

[wyldckat]

I've tested this just now with OpenFOAM 2.3.0 + ParaView 4.1.0 on Ubuntu 12.04 64-bit, installed from Deb package. What I get is shown in the first (left) attached image.

What fields do you have loaded in the "Volume Sections" on the lower left?

In addition, do you have any additional plug-ins loaded? From the menu, choose "Tools -> Manage plugins...". The second (right) image attached shows the default plug-ins that should be loaded.

[cfdopenfoam]

Originally Posted by wyldckat

What fields do you have loaded in the "Volume Sections" on the lower left?

In addition, do you have any additional plug-ins loaded? From the menu, choose "Tools -> Manage plugins...". The second (right) image attached shows the default plug-ins that should be loaded.

loaded fields: U.

i think no additional plug-ins are loaded. as attached.

and you may need click on the button "Toggle cell connectivity visibility" (shown in the third image) and sort the sheet by cell type. then you can see the pointIndex.

[wyldckat]

Originally Posted by cfdopenfoam

and you may need click on the button "Toggle cell connectivity visibility" (shown in the third image) and sort the sheet by cell type. then you can see the pointIndex.

Finally!!! I can see the issue now. That very small detail is something I wasn't looking for in the images and only when you finally wrote about it, did I finally manage to see it

OK, two details:

1. Yes, when the values are "-1" it means that the cells have fewer vertexes (points) due to their shape. Tetrahedrons only have 4 points, Pyramids only have 6, hexahedrons have 8.
2. If we run:

   checkMesh -region networkMesh

   It will tell us this:
   

   Overall number of cells of each type:
       hexahedra:     2140
       prisms:        0
       wedges:        0
       pyramids:      0
       tet wedges:    0
       tetrahedra:    0
       polyhedra:     30
       Breakdown of polyhedra by number of faces:
           faces   number of cells
               8   29
              10   1

   Therefore, there should only be hexahedrons and polyhedrons. The reason the others appear is because the decomposition of the polyhedrons was done automatically, because the "Use VTKPolyhedron" check box in the "Properties" widget is not checked.
   • For more details: http://openfoamwiki.net/index.php/FA...is_in_ParaView

[cfdopenfoam]

Originally Posted by wyldckat

• For more details: http://openfoamwiki.net/index.php/FA...is_in_ParaView

thanks very much, Bruno. this is exactly the problem. but, when i tried:

paraFoam -builtin -region networkMesh

or

paraFoam -region networkMesh -builtin

the -region networkMesh option seems not effective. so i test:

paraFoam -builtin

i got the very same result. both the commands give me the whole region with the error:

ERROR: In /home/yk/OpenFOAM/ThirdParty-2.3.0/ParaView-4.1.0/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 6524
vtkOpenFOAMReaderPrivate (0x3a347e0): Wrong list type for uniform field

and also, i got -1 pointIndex as the attached image shown.

any ideas?

best,
karelke

[wyldckat]

Quick answers:

Originally Posted by cfdopenfoam

so i test:

paraFoam -builtin

i got the very same result. both the commands give me the whole region with the error:

ERROR: In /home/yk/OpenFOAM/ThirdParty-2.3.0/ParaView-4.1.0/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 6524
vtkOpenFOAMReaderPrivate (0x3a347e0): Wrong list type for uniform field

Notice that the built-in reader with file extension ".foam" is able to select all regions from the same list of mesh items selection.

Originally Posted by cfdopenfoam

and also, i got -1 pointIndex as the attached image shown.

    Breakdown of polyhedra by number of faces:
        faces   number of cells
            8   29
           10   1

a cell with 10 faces means it possibly has somewhere between 10 and 12 points (vertexes), therefore there should be several columns from "Point Index 0" to "Point Index 11".
In the image is shown up to "Point Index 15", because you have loaded all mesh regions and there should be at least one polyhedral cell that has 16 vertexes (points).

[cfdopenfoam]

Originally Posted by wyldckat

Notice that the built-in reader with file extension ".foam" is able to select all regions from the same list of mesh items selection.

thanks for your hints, Bruno. hope this helps others.