CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Paraview & paraFoam

Paraview 3.98.0 does not update list of mesh regions

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   January 30, 2013, 10:20
Default Paraview 3.98.0 does not update list of mesh regions
  #1
Member
 
Marcus Letzel
Join Date: Sep 2012
Location: Aurich
Posts: 35
Rep Power: 6
letzel is on a distinguished road
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
letzel is offline   Reply With Quote

Old   January 30, 2013, 17:40
Default
  #2
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,635
Blog Entries: 39
Rep Power: 99
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings Marcus,

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

Best regards,
Bruno
__________________
wyldckat is offline   Reply With Quote

Old   January 31, 2013, 05:43
Default
  #3
Member
 
Marcus Letzel
Join Date: Sep 2012
Location: Aurich
Posts: 35
Rep Power: 6
letzel is on a distinguished road
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
letzel is offline   Reply With Quote

Old   January 31, 2013, 05:51
Default
  #4
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,635
Blog Entries: 39
Rep Power: 99
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
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
__________________
wyldckat is offline   Reply With Quote

Old   January 31, 2013, 06:32
Default
  #5
Member
 
Marcus Letzel
Join Date: Sep 2012
Location: Aurich
Posts: 35
Rep Power: 6
letzel is on a distinguished road
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
letzel is offline   Reply With Quote

Old   September 29, 2015, 05:47
Default
  #6
New Member
 
Join Date: Aug 2015
Posts: 17
Rep Power: 3
user10600 is on a distinguished road
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!

Last edited by user10600; September 29, 2015 at 08:17. Reason: Temporary solution found.
user10600 is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Update data in ParaView hpon OpenFOAM Paraview & paraFoam 18 May 10, 2015 14:55
how to set periodic boundary conditions Ganesh FLUENT 13 January 22, 2014 05:11
Update of the variables after dynamic mesh motion. gtg258f OpenFOAM Programming & Development 9 January 18, 2014 11:08
ParaView shows blocky mesh lfbarcelo OpenFOAM 3 June 25, 2010 08:16
problem of mesh of paraview sheintz OpenFOAM Paraview & paraFoam 1 September 14, 2009 11:27


All times are GMT -4. The time now is 11:48.