[Timm Feigel]

Dear all,

I need to locate a face in an OpenFOAM mesh by knowing its ID using Paraview. Although this seems possible for cells and points using the spread sheet option after splitting the view (see attached screenshot), it is not obvious to me how to do the same for faces.

Any help is highly appreciated, many thanks in advance.
Regards,
Timm

[ullal]

Timm,

Did you figure out how to do this, i had exactly the same problem

[Timm Feigel]

Originally Posted by ullal

Timm,

Did you figure out how to do this, i had exactly the same problem

Hello ullal!

No, unfortunately I haven't found a satisfying answer yet. In case I will, I will naturally post here for future readers.

Regards, Timm

[ViktorKL]

If there is no other way you can create a faceSet with topoSet and visualize it as VTK-format.

In a topoSet dictionary, you need to provide the Face-IDs in a list by using the labelToFace-source as in the following example:

    {
        name        zeroArea_f;
        type        faceSet;
        action      new;
        source      labelToFace;
        sourceInfo
        {
            value
            (
            339
            13055
            ...
            );
        }
    }

After executing topoSet you can convert the resulting faceSet (named "zeroArea_f" in the example) into a VTK with the help of foamToVTK.

foamToVTK -faceSet zeroArea_f

It will create a .vtk-file with the faceSet's name in a VTK folder of your OpenFOAM case repository. You can open this file in paraview and visualize the faces.

This is a cumbersone workaround. However, it works when there is no other option.