CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Meshing & Mesh Conversion

Problems after snappyHexMesh with paraview

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 2, 2015, 14:19
Default Problems after snappyHexMesh with paraview
  #1
New Member
 
Andreas V.
Join Date: Jul 2014
Posts: 13
Rep Power: 2
andreas0209@hotmail.com is on a distinguished road
Hi

I have a problem with my simulation case and I am still unexperienced enough to solve the problem. Hope you can help...

In my case I have a geometry which exist of different 5 stl files.
I have tested all my setting with a very coarse background mesh and only one single stl file (out of these 5).
Everything went (from my point of view) ok and the geometry looks quite ok after using snappyHexMesh.

Now I have excess to a supercomputer facility and prepared the case with a much finer mesh and all geometries. For the simulations I've used 80 processors for a parallel application (depomposePar). After the snappyHexMesh step I've looked into the log file of the meshing process the meshing report says that the mesh is ok.

And here is my problem.
If I try to open the meshed geometry in paraview (by using paraFoam in the case directory), paraview shows only the block mesh with the different patch names. I also tried to reconstruct the case (with reconstructParMesh), but with the same result.

What is wrong here. Any help is very much appreciated!

Thanks in advance
Andreas
andreas0209@hotmail.com is offline   Reply With Quote

Old   February 2, 2015, 16:47
Default
  #2
Senior Member
 
Matthew Denno
Join Date: Feb 2010
Posts: 137
Rep Power: 7
mgdenno is on a distinguished road
Just one quick thought, did you chose the option (dropdown) to view the decomposed case in paraview?
mgdenno is offline   Reply With Quote

Old   February 2, 2015, 17:11
Default
  #3
New Member
 
Andreas V.
Join Date: Jul 2014
Posts: 13
Rep Power: 2
andreas0209@hotmail.com is on a distinguished road
That was one of the problems. There was no option bottom (decompose/reconstruct).
andreas0209@hotmail.com is offline   Reply With Quote

Old   February 2, 2015, 17:14
Default
  #4
Senior Member
 
Matthew Denno
Join Date: Feb 2010
Posts: 137
Rep Power: 7
mgdenno is on a distinguished road
I am not at my computer but you might need to launch paraFoam -builtin to get that option.
mgdenno is offline   Reply With Quote

Old   February 3, 2015, 04:13
Default
  #5
New Member
 
Andreas V.
Join Date: Jul 2014
Posts: 13
Rep Power: 2
andreas0209@hotmail.com is on a distinguished road
Hi Matthew

thank you for the hint, but I have still the same problem.
I have attached the log file of this job (I needed to shrink it a bit...). It looks to me that everything is ok and I would expect that I am able to see the meshed parts in paraview. But I don't. I am a bit helpless. Does that mean that the meshing process failed or that there is only a visualisation problem?

File/case information:
In the log file there are all information from the blockMesh, decomposePar and snappyHexMesh step. I deletetd most of the snappy-output because of the file size limitation here. But there were not error/warnings or something.

After this process it worked not on paraview. Then I tried to run: reconstructParMesh, but with the same problem.

Thanks.

Andreas
Attached Files
File Type: txt OFjob1.txt (85.5 KB, 8 views)
andreas0209@hotmail.com is offline   Reply With Quote

Old   February 3, 2015, 04:23
Default
  #6
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,089
Rep Power: 19
alexeym will become famous soon enoughalexeym will become famous soon enough
Hi,

Take a look at your log:

Code:
...
    6	5084040
Writing mesh to time 3
Wrote mesh in = 1288.72 s.
...
as you ran snappyHexMesh without -overwrite flag it saved mesh from every iteration into different time folder. I.e. 0 is your blockMesh, 1 after first snappyHexMesh iteration, etc.
alexeym is offline   Reply With Quote

Old   February 5, 2015, 03:30
Default
  #7
New Member
 
Andreas V.
Join Date: Jul 2014
Posts: 13
Rep Power: 2
andreas0209@hotmail.com is on a distinguished road
Thanks.

This was really helpful. I understood what happened but still. The meshed stl file is not visible.

What I did now:
1. blockMesh
2. decomposed with "hierarchical"
3. snappyHexMesh -overwrite
4. reconstructParMesh

If I look into the logfile I cannot see any error warnings, problems, etc.

I am now completely hopeless.
andreas0209@hotmail.com is offline   Reply With Quote

Old   February 5, 2015, 03:39
Default
  #8
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,089
Rep Power: 19
alexeym will become famous soon enoughalexeym will become famous soon enough
If the sequence of commands you've posted is exact, then

1. You create mesh with blockMesh (let's call it (1))
2. Decompose mesh (1)
3. Run 'snappyHexMesh -overwrite', so it runs in serial regime and creates mesh in constant folder (let's call it (2)).
4. Run reconstructParMesh, so the mesh (1) is reconstructed over newly created (2).

Or step 3 was definitely run in parallel regime?
alexeym is offline   Reply With Quote

Old   February 5, 2015, 11:35
Default
  #9
New Member
 
Andreas V.
Join Date: Jul 2014
Posts: 13
Rep Power: 2
andreas0209@hotmail.com is on a distinguished road
Yes this is correct.
Is it a problem that I use first blockMesh and then decomposePar and the rest?


Or is it important to decompose first and then doing blockMesh, snappyHexMesh?

And yes I am sure that I have run this case in parallel!
andreas0209@hotmail.com is offline   Reply With Quote

Old   February 5, 2015, 11:47
Default
  #10
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,089
Rep Power: 19
alexeym will become famous soon enoughalexeym will become famous soon enough
Everything became rather complicated

1. You say that you run commands exactly as it was written 'snappyHexMesh -overwrite'. This command runs snappyHexMesh in serial mode, to run it in parallel you should do 'snappyHexMesh -overwrite -parallel'

2. You're definitely sure about running the case in parallel.

In the log you have attached to the previous message it was clear that snappyHexMesh was run in parallel regime. But I don't see the log this time, it's difficult to say what has been happened.
alexeym is offline   Reply With Quote

Old   February 23, 2015, 12:00
Default Problem solved
  #11
New Member
 
Andreas V.
Join Date: Jul 2014
Posts: 13
Rep Power: 2
andreas0209@hotmail.com is on a distinguished road
Hi alexeym

thank you again for kicking my a..

I finally solved the problem with you help. I used either -overwrite or -parallel but not -overwrite -parallel.
I used the following commands:
blockMesh > log.block
surfaceFeatureExtract
topoSet
decomposePar -force
mpiexec_mpt snappyHexMesh -overwrite -parallel

Thanks again.

Andreas
andreas0209@hotmail.com is offline   Reply With Quote

Reply

Tags
openfoam 2.3.1, parafoam, snappyhexmesh 3d

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
snappyHexMesh - 2D Cylinder Problems Logan Page OpenFOAM Native Meshers: snappyHexMesh and Others 4 May 27, 2013 12:07
paraview installation woes vex OpenFOAM Installation 15 January 30, 2011 08:11
Installation problems about Paraview and PV3foamreader clark_liang OpenFOAM Installation 1 January 12, 2009 07:05
Problems using paraview 244 under open FOAM 141 or 13 sergio OpenFOAM Paraview & paraFoam 0 March 13, 2008 14:52
Problems with paraView alejo OpenFOAM Pre-Processing 0 February 17, 2006 08:24


All times are GMT -4. The time now is 03:28.