[jms]

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

[elisabet]

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 GUI
-Cache Mesh
-Extrapolate Walls
-Include Sets
-...

just click on 'Include Sets' and you'll see it.


If you prefer dealing with paraview, use the command:

foamToVTK -cellSet highAspectRatioCells

and load the file as usual.



enjoy!

elisabet

[jms]

Thank you very much for your help!

What about this other thread I started in here?... do you know any thing?

Gràcies!

José

[idefix]

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

[wyldckat]

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:

checkMesh -allGeometry -allTopology

Best regards,
Bruno

[idefix]

Hello Bruno,

thanks for your help.

checkMesh that´s that everything is ok

but checkMesh -allGeometry -allTopology

says:

Cell determinant (wellposedness) : minimum: 0 average: 0
***Cells with small determinant found, number of cells: 4680
<<Writing 4680 under-determined cells to set underdeterminedCells
Concave cell check OK.

Failed 1 mesh checks.

End

It´s a test case and therefore the grid is very small. It has only 4680 cells - so every cell is "damaged".

But what does it exactly mean?

Thanks a lot
Regards
Idefix

[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

[wyldckat]

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":

foamToVTK -cellSet underdeterminedCells

Only because you got this message:

<<Writing 4680 under-determined cells to set underdeterminedCells

Best regards,
Bruno

[Sherlock_1812]

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?

[wyldckat]

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

[Sherlock_1812]

Thank you Bruno.

[miladrakhsha]

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.

[wyldckat]

Greetings miladrakhsha,

Regarding the first question, if you're using OpenFOAM 2.x:

paraFoam -builtin

If you're using foam-extend:

paraFoam -nativeReader

Regarding the second question, without knowing how exactly which versions of OpenFOAM you're using and which ParaView versions, the best answer I can come up quickly is to point you to this post: http://www.cfd-online.com/Forums/ope...tml#post345619 - post #2

Best regards,
Bruno