|
[Sponsors] |
[OpenFOAM] Visualizing checkMesh results in Paraview |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
June 25, 2013, 12:58 |
Visualizing checkMesh results in Paraview
|
#1 |
New Member
Claudio
Join Date: May 2010
Location: Boston, MA
Posts: 28
Rep Power: 15 |
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 |
|
June 26, 2013, 04:43 |
|
#2 |
Senior Member
|
Hi Claudio,
You can use the foamToVTK utility to make VTK files of any set: Code:
foamToVTK -faceSet nonOrthoFaces -time 0 Regards, Tom |
|
June 22, 2016, 08:41 |
|
#3 |
New Member
Madeleine
Join Date: Jun 2016
Posts: 14
Rep Power: 9 |
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 |
|
June 22, 2016, 09:03 |
|
#4 |
Senior Member
|
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 |
|
June 22, 2016, 09:23 |
|
#5 |
New Member
Madeleine
Join Date: Jun 2016
Posts: 14
Rep Power: 9 |
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. |
|
June 22, 2016, 09:29 |
|
#6 |
Senior Member
|
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 Regards, Tom |
|
June 23, 2016, 01:50 |
|
#7 |
New Member
Madeleine
Join Date: Jun 2016
Posts: 14
Rep Power: 9 |
Hi Tom
it worked. Thank you |
|
July 13, 2016, 05:53 |
|
#8 |
New Member
Christine
Join Date: Jan 2016
Posts: 1
Rep Power: 0 |
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 |
|
July 13, 2016, 06:30 |
|
#9 |
Senior Member
|
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 |
|
September 11, 2017, 10:30 |
|
#10 | |
New Member
Umer
Join Date: Aug 2016
Posts: 29
Rep Power: 9 |
Quote:
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 |
||
September 11, 2017, 12:02 |
|
#11 |
Senior Member
|
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 |
|
September 12, 2017, 05:49 |
|
#12 | |
New Member
Umer
Join Date: Aug 2016
Posts: 29
Rep Power: 9 |
Quote:
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 |
||
September 12, 2017, 06:06 |
|
#13 |
Senior Member
|
Hi,
I would suggest to use: Code:
foamToVTK -cellSet <cellSetName> -latestTime You can than visualize the VTK file that follows from this. I do not think there is another option. Regards, Tom |
|
September 12, 2017, 07:30 |
|
#14 | |
New Member
Umer
Join Date: Aug 2016
Posts: 29
Rep Power: 9 |
Quote:
Thanks again . umer |
||
September 19, 2017, 04:31 |
|
#15 |
Senior Member
matej forman
Join Date: Mar 2009
Location: Brno, Czech Republic
Posts: 182
Rep Power: 17 |
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. |
|
July 21, 2020, 13:58 |
updated method for openfoam 7
|
#16 | |
Member
Join Date: Feb 2016
Posts: 41
Rep Power: 10 |
Quote:
in openfoam 7 we can now execute checkMesh with the writeSets option. Code:
checkMesh -writeSets <output file type> so if you want to go to paraview (like most ppl) then do this to get the vtk output Code:
checkMesh -writeSets vtk |
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Regarding regIOobjectRead.C at line 73 error while converting results to paraview | hhh | OpenFOAM Post-Processing | 5 | November 24, 2016 02:45 |
use paraview to visualize the openfoam output results | hz283 | OpenFOAM | 2 | July 23, 2013 08:18 |
[General] Importing 1D Tecplot files to Paraview with Zones results in NA | weirdtunguska | ParaView | 2 | July 18, 2013 11:01 |
Visualize checkMesh output with Paraview | Horus | OpenFOAM | 1 | May 29, 2012 11:51 |
viewing probe results with Paraview | feldy77 | OpenFOAM | 0 | November 2, 2011 19:31 |