[Ryan.]

Hi,

is there any OpenFOAM function object similar to surfaceSampling but for the volume? I want to sample a volume region or the whole domain on the run. I don't want to do the reconstruction as it's time-consuming and I am only interested in a small region near the outlet.

thanks in advance,
Ryan

[tomf]

Hi,

I am not sure what you exactly want to do, but maybe the volFieldValue functionObject is of help?

It uses a volRegion for doing some stuff.

This means you would need a cellSet or cellZone and then probably you need to specify whatever you need in the volFieldValue part.

I am not sure what the limitations are. Maybe you can make a small case to experiment on.

Good luck,
Tom

[zhangyan]

Maybe you can try this:
https://github.com/StachuraMichal/Op...sampleCellZone

[Ryan.]

Originally Posted by zhangyan

Maybe you can try this:
https://github.com/StachuraMichal/Op...sampleCellZone

Thanks a lot. This is precisely what I was looking for. The only issue is that it only writes the points to the file but doesn't write the mesh. Do you know how to append the mesh to the samples?

[lukasf]

Hi Ryan,


have you found a solution to sample volumes and to visualize those with paraview?


Happy for any help.


Lukas

[al.csc]

Originally Posted by lukasf

Hi Ryan,


have you found a solution to sample volumes and to visualize those with paraview?


Happy for any help.


Lukas

Here an example for ESI version:

functions
{
    type    sets;
    libs    (sampling);
    log     on;
    enabled true;

    writeControl    timeStep;
    writeInterval   1;
    setFormat       raw; //or vtk for Paraview
    interpolationScheme cell;
    fields ( U );
    sets
    (
        centres
        {
            type    cellCentre;
           bounds  (0 0 0) (0.1 0.1 0.1);
        }
    );
}

Paste it at the end of your controlDict and adjust it for your case.

Cheers!

[lukasf]

Originally Posted by al.csc

Here an example for ESI version:

functions
{
    type    sets;
    libs    (sampling);
    log     on;
    enabled true;

    writeControl    timeStep;
    writeInterval   1;
    setFormat       raw; //or vtk for Paraview
    interpolationScheme cell;
    fields ( U );
    sets
    (
        centres
        {
            type    cellCentre;
           bounds  (0 0 0) (0.1 0.1 0.1);
        }
    );
}

Paste it at the end of your controlDict and adjust it for your case.

Cheers!

Hi Ryan,


thank you.

I works. However, when I want to visualize the .vtk files with ParaView I do not like the way the file is displayed. Somehow, it only consists out of points.

Hence, I prefer this way:

    volFieldValue1
    {
        type                volFieldValue;
        libs                 ("libfieldFunctionObjects.so");
        log                  false; //true;
        writeControl adjustableRunTime;
        writeFormat     ascii; //binary;
        writeInterval 1e-5;
        writeFields       true;//writes the fields of the volume
        //timeStart       0;
        //timeEnd         1000;
        regionType       cellSet; //cellZone;
        name               box; // box is the cellSet or cellZone defined by the topoSetDict
        operation         none; 
        fields
        (
            U T p
        );
    }

However, this code did not work for the ESI version v1912. The fields where just empty. However, using version V2112 (same code) results in all values written into the files.

One receives a file in postProcessing/volFieldValue1 which is not important.
The volume field is directly written to the time directories or time directories of the processor0.

In this directory I run this command.

                         foamToVTK -cellSet box -useTimeName -excludePatches '(".*")' -noFaceZones

This way I get .vtk files which are visualized more nicely in ParaView.
Moreover, I source a non ESI openfoam Version for the foamToVTK command because this way the "-useTimeName" is available which I prefer.