I want to visualize my OpenFOAM simulation results with ParaView but I'm confused, which version should I use ?

FAQ
1

Short Answer:

  • go to paraview.org/download
  • download the last version of ParaView available
  • Use it to visualize your results

Long Answer:

OpenFOAM ships with a script named paraFoam, which can be used
to call ParaView with custom OpenFOAM-specific reader modules, as well
as with the standard reader that comes with ParaView/VTK.

As stated in the OpenFOAM wiki, There is almost no reason to use these
particular reader modules instead of the official binary release.

Also, this discourse cannot help with questions about the so-called
paraFoam modules whatsoever, since these reader modules are developed
independently from ParaView.

Note that some versions of the paraFoam script may contain a somewhat
confusing statement:

The official reader module for OpenFOAM data does not exist on
your system. This means that the version of ParaView you are using
was not compiled with OpenFOAM, or distributed with a packaged version
of OpenFOAM.

If you are in the habit of using paraFoam as a command (eg, since it
touches a file into existence), simply use paraFoam -vtk or paraFoam -builtin instead. Use a shell alias.

2 Likes
2

In addition to @mwestphal comments, please note that for the long term OpenCFD (www.openfoam.com) would prefer to focus efforts into extending and improving the ParaView/VTK readers for OpenFOAM and eventually be able to fully deprecate the reader module behind paraFoam.

Here is the current score sheet (Jul-2022) - taken from the OpenFOAM wiki:

Do I really need the ParaView plugins?

Before blindly launching into compiling ParaView with the idea that this is simply necessary for a complete software stack, you should examine your actual requirements. Note that the term paraFoam is often used loosely to mean the reader plugins, but it is merely a small wrapper script.

Native reader OpenFOAM Plugin Functionality
[+] [-] Does not require OpenFOAM installation
[+] [-] No duplicate of the OpenFOAM mesh in memory
[+] [-] Supports decomposed cases (without reconstructPar)
[+] [-] Supports parallel rendering
[-] [+] Handles collated file formats
[-] [+] Selection of faceSet, faceZones, etc.
[paraview-5.10] [+] Patch group selection - merged
[paraview-5.10] [+] Dimensioned (Internal) fields - merged
[in progress] [+] finiteArea mesh and results - merged, but inactive
[-] [+] Additional patch names (low priority)

Workarounds:

  • Use foamToVTK for faceSets, faceZones as required and load the generated VTK files in ParaView as usual.
Native reader blockMeshDict Plugin Functionality
n/a [+] Explore block structures

Alternatives:

  • Use blockMesh -write-vtk to generate the block topology as a VTK file that can be explored in ParaView as required.
    The ParaView Hover Points On function is particularly useful!
1 Like