CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM Paraview & paraFoam (
-   -   Paraview 3.98.0 does not update list of mesh regions (

letzel January 30, 2013 10:20

Paraview 3.98.0 does not update list of mesh regions
Dear Foamers,

since my upgrade from Paraview 3.14.1 to 3.98.0, a useful Paraview feature seems to be missing. Paraview 3.98.0 does not update the list of mesh regions any more. I define "update" in a sense that if a later time step has more mesh regions than the initial time step "0", the new regions should be added to the list of mesh regions. Paraview 3.14.1 does this as expected, while 3.98.0 does not.

This feature is relevant for me because I am importing geometry with snappyHexMesh. The imported geometry does not yet shop up at the initial time step "0".

My LES workflow is a bit special because I have a modified piso solver with y as vertical axis, but my Blender-generated STL input data have z as vertical axis, and because I execute both snappyHexMesh and the modified solver in parallel:

blockMesh > blockMesh.log 2>&1
decomposePar -force > decomposePar1.log 2>&1
foamJob -parallel snappyHexMesh
foamJob -parallel checkMesh -latestTime
reconstructParMesh -latestTime -mergeTol 1e-06
transformPoints -yawPitchRoll "(0 0 -90)"
transformPoints -translate "(0 0 6)"
cp -p 0/* 0.02
setFields -latestTime
decomposePar -force > decomposePar2.log 2>&1
foamJob -parallel pisoMod
decomposePar -constant

Although Paraview 3.98.0 correctly recognizes the updated internal mesh based on the contents of the processor*/0.02/polyMesh subdirectories, the imported geometry is not added to the list.

Has anybody else observed this behaviour? Do you have a suggestion how to solve or avoid this problem? Looking forward to receive your feed-back.

Best regards,

wyldckat January 30, 2013 17:40

Greetings Marcus,

Which file reader are you using? The internal reader in ParaView or OpenFOAM's own plugin reader for ParaView?

Best regards,

letzel January 31, 2013 05:43

Dear Bruno,

I am not using paraFoam, which would generate a temporary .OpenFOAM stub file but would not offer the "case type" choice "decomposed case".

Instead, following the thread decomposed case reader in Paraview,I generate a .foam stub file and open it with paraview, or paraFoam -builtin. So it is the built-in reader which I am using. This reader offers to read decomposed data directly.

My Paraview version is ParaView-3.14.1-Win64-x86.

Best regards,

wyldckat January 31, 2013 05:51

Hi Marcus,

Have you tried Takuya's up-to-date plug-in? You can get it for Windows from here:

Best regards,

letzel January 31, 2013 06:32

Hi Bruno,

very good suggestion. I have just installed Takuya's plug-in, and it solves my problem. It even offers a convenient way to rescan the timesteps.

Thank you very much!

user10600 September 29, 2015 05:47


I have a similar problem with Paraview 3.98.1.
I only obtain in the "Mesh Regions" the Regions from the Block Mesh, even though I am using, after Block Mesh, the utilities Snappy Hex Mesh and Topo Set followed by Extrude To Region Mesh.

Is there another way to "update" the Mesh Regions in Paraview 3.98.1 without installing an add-on ?

Thanks in advance.

EDIT : I found a way to get what I wanted to obtain.
After running blockMesh, I got a "boundary" file in the constant/polyMesh folder. After running snappyHexMesh, I also got a "boundary" file but in the the folder "time step in which the snappy writes the mesh"/polyMesh.
I then just substitute the first "boundary" file in the constant folder with the new one from the snappy.
It also works with regions that you create with topoSet and extrudeToRegionMesh.
Now I am able to see in Paraview the new Mesh Regions.

Be careful though with the first time step in Paraview, it might eventually directly crash. Just put a later time step.
I know that this method looks kinda ugly ^^.. but I hope it will help someone!

All times are GMT -4. The time now is 19:21.