High Aspect Ratio Cells in Paraview
Dear all,
Do any of you know how to check the cells with highest aspect ratio with Paraview? If there are cells with high aspect ratio checkMesh from OpenFOAM creates a file in "constant/sets" called "highAspectRatioCells". Is there any way to open this one in Paraview? Thanks. Regards, José |
Hi José,
Of course there is! If you open your case with paraFoam, at the main page you see a list of options, among them: -Update GUIjust click on 'Include Sets' and you'll see it. If you prefer dealing with paraview, use the command: foamToVTK -cellSet highAspectRatioCellsand load the file as usual. enjoy! elisabet |
Thank you very much for your help!
What about this other thread I started in here?... do you know any thing? Gràcies! José |
Hello,
foamToVTK -cellSet highAspectRatioCells is not working in my case. I get the error massage: --> FOAM FATAL ERROR: Cannot find file "" in directory "polyMesh/sets" in times 0 down to constant From function Time::findInstance(const fileName&, const word&, const IOobject::readOption, const word&) in file db/Time/findInstance.C at line 140. FOAM exiting What is wrong? Can somebody help me? Thanks a lot |
Greetings idefix,
Did you run checkMesh? Did it report any high aspect ratio cells? You might also want to try the full diagnosis, by running: Code:
checkMesh -allGeometry -allTopology Bruno |
Hello Bruno,
thanks for your help. checkMesh that´s that everything is ok but checkMesh -allGeometry -allTopology says: Quote:
But what does it exactly mean? Thanks a lot Regards Idefix |
Hello again,
I just try a little and was wondering about the error massage because the grid looks nice to me. By accident the error massage disappeared when I add more cells in the third dimension. Before the grid has only 1 cell in the third dimension. Why is this command (foamToVTK -cellSet highAspectRatioCells) not working for a 2d grid? Thanks a lot Idefix |
Hi Idefix,
You cannot get foamToVTK to process "highAspectRatioCells", simply because checkMesh did not find any cells with high aspect ratio. What you could have done when you got the error for "under-determined cells", is use foamToVTK to give you a VTK file for the cellSet named "underdeterminedCells": Code:
foamToVTK -cellSet underdeterminedCells Quote:
Bruno |
Check if all cells have an aspect ratio of 1?
Hi all,
I have a mesh that checkMesh has certified to be OK. Maximum aspect ratio is reported as 1.9. I would like to confirm if this aspect ratio is not in my region of interest where i'd like all cells to have an aspect ratio close to 1. So for a correct mesh, can I still view aspect ratio of all cells in paraView? And maybe plot the variation of aspect ratio along x-direction? |
Greetings Srivaths,
Although it would be very useful to get checkMesh to write out all of the fields calculated for mesh characteristics, unfortunately there isn't one in OpenFOAM by default, nor am I aware of any community source code utility that does this. Nonetheless, if you're interested in creating such an utility, have a look into the method "Foam::primitiveMeshTools::cellClosedness": https://github.com/OpenFOAM/OpenFOAM...shTools.C#L217 By the way, Github has a nice feature of searching for code inside the repository, by using the search edit box on the top of the page, so it's easy to find out which methods are calling this one! Best regards, Bruno |
Thank you Bruno.
|
Hi,
I am working with paraView 3.14.1 but seems like there is no include set option available. Any idea? Also, is there anyway I can change the version of paraview that I want to open the case with ? I have two versions of paraView and I would like to use the older version for post-processing even when I am using the new version of OpenFOAM which is by default associated with the newer version of paraView. |
Greetings miladrakhsha,
Regarding the first question, if you're using OpenFOAM 2.x: Code:
paraFoam -builtin Code:
paraFoam -nativeReader Best regards, Bruno |
All times are GMT -4. The time now is 21:38. |