CFD Online Discussion Forums - [OpenFOAM] Paraview 3.98.0 does not update list of mesh regions

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- ParaView (https://www.cfd-online.com/Forums/paraview/)

- - [OpenFOAM] Paraview 3.98.0 does not update list of mesh regions (https://www.cfd-online.com/Forums/paraview/112524-paraview-3-98-0-does-not-update-list-mesh-regions.html)

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:

Code:

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,
Marcus

Greetings Marcus,

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

Best regards,
Bruno

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,
Marcus

Hi Marcus,

Have you tried Takuya's up-to-date plug-in? You can get it for Windows from here: http://code.google.com/p/unofficial-...s#Installation

Best regards,
Bruno

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!
Marcus

Hi,

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!

Refreshing Mesh Regions and Cell Arrays Lists

Hello,

I think my question is related to this thread. I usually save my visualizations as states to preserve the filter pipeline and all its settings. If I rename patches, their quantity changes or if field arrays get added or removed, the old ones still appear in the lists labeled "Mesh Regions" and "Cell Arrays", see picture. I also often use an existing state as a template and copy it to be used with another case, ending up showing lots of unused and not-existing boundary patches or fields in the lists. Is there any way how they can be updated to reflect the actual state of data present in the OpenFOAM case files?

Clicking the "Refresh" button or executing "Reload Files" doesn't update the lists. The only workaround I've found so far is to open the *.pvsm xml files, search for known boundary and field names, deleting all the entries manually and saving. When the state is then loaded again, boundary patches and fields get read from the case files and are up-to-date. I also couldn't find any info about this in the ParaView forum. I use ParaView for macOS and this has persisted from version 5.7 up to the current 5.9.

Thanks for any hints!

Cheers, Claudio