[Gearb0x]

Hi

I have a case which is decomposed using the "metis" method.

How can I see the different parts of the mesh? And their results?
I tried to run parafoam in the case/processor0 directory but it didn't work.

Thanks for your help.

[erklaerbaer]

I am not familiar with the "metis" method but did you try "reconstructPar" to get your results back together?

[Gearb0x]

Hello,

Thanks for your answer. In fact getting the cases back together is, indeed, done by typing 'reconstructPar' but what I would to are the part separated and not together To see how the mesh was separated.

By curiosity, How do you use the other methods (other than metis) ? Do you have a tutorial or something?

Thanks for your help

[erklaerbaer]

Perhaps this helps you http://www.openfoamworkshop.org/2009...InParallel.pdf.

Till now i just used simple and was able to start Paraforam in the "processorX" folder, maybe paraFoarm cant handle the way metis splits up the Mesh

You could try "foamToVTK" an then paraview but thats just a guess.
Perhaps simpleViewer can also help you, but a am not shure what file it reads for showing the mesh.

[Gearb0x]

Again, Thanks for the help!

But it's strange that paraFoam can't handle this

[wyldckat]

Greetings Gearb0x and erklaerbaer,

Uhm, I just read diagonally the pdf from the link that Andreas has posted, and I found on the penultimate page:

When post-processing cases that have been run in parallel the user has two options:
• reconstruction of the mesh and field data to recreate the complete domain and fields, which can be post-processed as normal;
• post-processing each segment of decomposed domain individually;

Although it doesn't specifically say how, and I haven't tested this right now, but my guess is that if you execute paraFoam at the base folder of the case, the PV3FoamReader plugin will detect the processor partitions and allow you to see them independently, by picking them from the list, just as the fields!

By the way, just in case the snapshot "0 seconds" doesn't show anything, try the next snapshot... I have had problems in the past with the first snapshot in single core runs, due to some discrepancy between meshes or boundaries or something like that

Best regards,
Bruno

[herbert]

Hi,

just type "paraFoam -case processorX" to see only the result of processor X.

Good luck
Stefan

[f0208secretx]

Hi,

I want to visualize the master mesh after running parallelized snappyHexMesh, so I use the utility reconstructParMesh

 reconstructParMesh -mergeTol 1E-6 -time 0

and yet I keep getting the error

 --> FOAM FATAL ERROR: 
No times selected

    From function reconstructParMesh
    in file reconstructParMesh.C at line 578.

FOAM exiting

I can see the individual mesh without any problem. I can also resemble the master mesh in paraview by loading all of them in. So really I was just wondering why this doesn't work as opposed to desperately trying to get it work. Thanks for any advise anyway.



JHW

[Bernhard]

I see this thread is quite old, but I wrote a script a time ago that might help you.

Step 1. Create .foam files in all directories

#!/bin/bash
for dd in `find -name 'proc*' -type d`
do 
 echo $dd
 cd $dd
 echo $PWD
 touch `basename $PWD`".foam"
 cd ..
done

Step 2. Run the following Python script from the Paraview Python shell (some user input in the source is not automated)

try: paraview.simple
except: from paraview.simple import *
paraview.simple._DisableFirstRenderCameraReset()

import random

procs = 64
for proc in range(procs):
 print proc
 foamfile='case/processor'+str(proc)+'/processor'+str(proc)+'.foam' 
 processor0_foam = OpenFOAMReader(FileName = foamfile)

 processor0_foam.CellArrays = []
 processor0_foam.LagrangianArrays = []
 processor0_foam.MeshRegions = ['internalMesh']
 processor0_foam.PointArrays = []
 processor0_foam.CellArrays = []
 mr0 = GetDisplayProperties(processor0_foam)
 #mr0.DiffuseColor = [1, 1, float(proc)/float(procs-1)]
 mr0.DiffuseColor = [random.random(), random.random(), random.random() ]
 RenderView1 = GetRenderView()
 DataRepresentation2 = Show()

Render()

I hope someone can use these scripts

[qutadah.r]

Originally Posted by herbert

Hi,

just type "paraFoam -case processorX" to see only the result of processor X.

Good luck
Stefan

I cannot run paraFoam, I have a problem with paraview and I am not root user to fix it.. Any alternative?


I am also using OptimisationSwitches and fileHandler in my controlDict and it grouped all processors in a single processor, "processors96". So how do I see the decomposed mesh in this case?


I have also seen the option "Case Type" inside paraview in properties panel when importing a case, it has both reconstructed and Decomposed case as options. I have tried decomposed but still whole mesh is there, not sure where to activate only a specific processor. Any idea?





Thanks !

[ghastbug]

Personally I can't use the paraFoam command, but I installed paraview on windows and run it without using the shell. If parafoam gives you problem you might be able to install paraview and use it normally instead.


Also, on the topic of decomposed cases: paraview has an option to render decomposed cases instead of deconstructed cases, so you don't even need to use reconstructPar

[qutadah.r]

The thing is, I can run paraview, but I cant use the paraFoam command. I can run paraview xx.foam or just import cases in there, but there is a problem which is quite known that has a fix but I cant because im not root user, so I cannot use paraFoam.


But the thing is, even when importing a case and I saw the option decomposed mesh or reconstructed, but how can I even choose which processor? I cant seem to find that....


Thanks @ghastbug