Visualizing checkMesh results in Paraview
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 |
Hi Claudio,
You can use the foamToVTK utility to make VTK files of any set: Code:
foamToVTK -faceSet nonOrthoFaces -time 0 Regards, Tom |
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 |
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 |
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. |
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 |
Hi Tom
it worked. Thank you :) |
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 |
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 |
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 |
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 |
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 |
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 |
Quote:
Thanks again . umer |
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. |
updated method for openfoam 7
Quote:
in openfoam 7 we can now execute checkMesh with the writeSets option. Code:
so if you want to go to paraview (like most ppl) then do this to get the vtk output Code:
|
All times are GMT -4. The time now is 03:57. |