CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Paraview & paraFoam

Visualizing checkMesh results in Paraview

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree18Likes
  • 18 Post By tomf

Reply
 
LinkBack Thread Tools Display Modes
Old   June 25, 2013, 12:58
Default Visualizing checkMesh results in Paraview
  #1
New Member
 
Claudio
Join Date: May 2010
Location: Boston, MA
Posts: 28
Rep Power: 9
Claudio is on a distinguished road
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

Code:
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
Claudio is offline   Reply With Quote

Old   June 26, 2013, 04:43
Default
  #2
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Delft, Netherlands
Posts: 359
Rep Power: 14
tomf is on a distinguished road
Send a message via MSN to tomf Send a message via Skype™ to tomf
Hi Claudio,

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

Code:
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
kiddmax, Claudio, risku9 and 15 others like this.
tomf is offline   Reply With Quote

Old   June 22, 2016, 08:41
Default
  #3
New Member
 
Madeleine
Join Date: Jun 2016
Posts: 14
Rep Power: 2
Madi is on a distinguished road
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
Madi is offline   Reply With Quote

Old   June 22, 2016, 09:03
Default
  #4
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Delft, Netherlands
Posts: 359
Rep Power: 14
tomf is on a distinguished road
Send a message via MSN to tomf Send a message via Skype™ to 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
tomf is offline   Reply With Quote

Old   June 22, 2016, 09:23
Default
  #5
New Member
 
Madeleine
Join Date: Jun 2016
Posts: 14
Rep Power: 2
Madi is on a distinguished road
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.
Madi is offline   Reply With Quote

Old   June 22, 2016, 09:29
Default
  #6
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Delft, Netherlands
Posts: 359
Rep Power: 14
tomf is on a distinguished road
Send a message via MSN to tomf Send a message via Skype™ to 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
Code:
flattenMesh
utility.

Regards,
Tom
tomf is offline   Reply With Quote

Old   June 23, 2016, 01:50
Default
  #7
New Member
 
Madeleine
Join Date: Jun 2016
Posts: 14
Rep Power: 2
Madi is on a distinguished road
Hi Tom

it worked. Thank you
Madi is offline   Reply With Quote

Old   July 13, 2016, 05:53
Default
  #8
New Member
 
Christine
Join Date: Jan 2016
Posts: 1
Rep Power: 0
Tanne25 is on a distinguished road
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
Tanne25 is offline   Reply With Quote

Old   July 13, 2016, 06:30
Default
  #9
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Delft, Netherlands
Posts: 359
Rep Power: 14
tomf is on a distinguished road
Send a message via MSN to tomf Send a message via Skype™ to 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
tomf is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
How to load all <case>/surfaces/*/*.vtk at once into Paraview holodeck10 OpenFOAM Paraview & paraFoam 7 September 15, 2015 07:18
viewing probe results with Paraview feldy77 OpenFOAM 0 November 2, 2011 20:31
Visualizing in Paraview Kvadar OpenFOAM Paraview & paraFoam 5 July 25, 2011 03:36
Segmentation fault when visualizing in ParaView fsalvucci OpenFOAM 9 July 30, 2010 15:39
Visualizing face normals in ParaView nikunj OpenFOAM Paraview & paraFoam 0 April 18, 2006 01:30


All times are GMT -4. The time now is 13:41.