CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Paraview & paraFoam (http://www.cfd-online.com/Forums/openfoam-paraview/)
-   -   turbineSiting tutorial and paraview-3.98.0 (http://www.cfd-online.com/Forums/openfoam-paraview/122678-turbinesiting-tutorial-paraview-3-98-0-a.html)

pajot August 25, 2013 13:20

turbineSiting tutorial and paraview-3.98.0
 
After successfully running the Allrun script in the simpleFoam/turbineSiting tutorial, paraview won't play the simulation.

(Note that in the below, paraFoam is an alias to 'paraFoam -builtin'. Without '-builtin', paraFoam won't even run.)

Code:

../turbineSiting $ paraFoam
created temporary 'turbineSiting.foam'
ERROR: In /var/tmp/portage/sci-visualization/paraview-3.98.0/work/ParaView-3.98.0-src/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 6535
vtkOpenFOAMReaderPrivate (0x386d430): Wrong list type for uniform field


ERROR: In /var/tmp/portage/sci-visualization/paraview-3.98.0/work/ParaView-3.98.0-src/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 6535
vtkOpenFOAMReaderPrivate (0x386d430): Wrong list type for uniform field


ERROR: In /var/tmp/portage/sci-visualization/paraview-3.98.0/work/ParaView-3.98.0-src/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 6535
vtkOpenFOAMReaderPrivate (0x386d430): Wrong list type for uniform field


ERROR: In /var/tmp/portage/sci-visualization/paraview-3.98.0/work/ParaView-3.98.0-src/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 6535
vtkOpenFOAMReaderPrivate (0x386d430): Wrong list type for uniform field


ERROR: In /var/tmp/portage/sci-visualization/paraview-3.98.0/work/ParaView-3.98.0-src/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 6535
vtkOpenFOAMReaderPrivate (0x386d430): Wrong list type for uniform field


ERROR: In /var/tmp/portage/sci-visualization/paraview-3.98.0/work/ParaView-3.98.0-src/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 6535
vtkOpenFOAMReaderPrivate (0x386d430): Wrong list type for uniform field


ERROR: In /var/tmp/portage/sci-visualization/paraview-3.98.0/work/ParaView-3.98.0-src/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 6535
vtkOpenFOAMReaderPrivate (0x386d430): Wrong list type for uniform field


ERROR: In /var/tmp/portage/sci-visualization/paraview-3.98.0/work/ParaView-3.98.0-src/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 6535
vtkOpenFOAMReaderPrivate (0x386d430): Wrong list type for uniform field


ERROR: In /var/tmp/portage/sci-visualization/paraview-3.98.0/work/ParaView-3.98.0-src/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 6535
vtkOpenFOAMReaderPrivate (0x386d430): Wrong list type for uniform field


ERROR: In /var/tmp/portage/sci-visualization/paraview-3.98.0/work/ParaView-3.98.0-src/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 6535
vtkOpenFOAMReaderPrivate (0x386d430): Wrong list type for uniform field


ERROR: In /var/tmp/portage/sci-visualization/paraview-3.98.0/work/ParaView-3.98.0-src/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 6535
vtkOpenFOAMReaderPrivate (0x386d430): Wrong list type for uniform field


ERROR: In /var/tmp/portage/sci-visualization/paraview-3.98.0/work/ParaView-3.98.0-src/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 6535
vtkOpenFOAMReaderPrivate (0x386d430): Wrong list type for uniform field


ERROR: In /var/tmp/portage/sci-visualization/paraview-3.98.0/work/ParaView-3.98.0-src/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 6535
vtkOpenFOAMReaderPrivate (0x386d430): Wrong list type for uniform field


ERROR: In /var/tmp/portage/sci-visualization/paraview-3.98.0/work/ParaView-3.98.0-src/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 6535
vtkOpenFOAMReaderPrivate (0x386d430): Wrong list type for uniform field


ERROR: In /var/tmp/portage/sci-visualization/paraview-3.98.0/work/ParaView-3.98.0-src/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 6535
vtkOpenFOAMReaderPrivate (0x386d430): Wrong list type for uniform field

I'm running OF 2.2.1. Although I've seen this error before, running 'paraFoam -builtin' addressed it the last time, and paraview-3.98.0 still works with my other simulation.

wyldckat August 25, 2013 14:50

Greetings Stephen,

The internal ".foam" reader is allergic to the boundary condition "uniformFixedValue". Therefore, before running paraview, you'll need to run this command:
Code:

sed -i -e "s=uniformFixedValue=fixedValue=g" [0-9][0-9]*/{U,p,k,nut,epsilon}
It will replace all occurrences of "uniformFixedValue" with "fixedValue", for all of the essential field files in the time folders after "0".

The problem is that you should not use these time folders for continuing the simulation afterwards, since this hack could damage the simulation characteristics for continuing simulating. But it should not damage the results for post-processing.

edit: By the way, the same happens in ParaView 3.12.0.

Best regards,
Bruno

pajot August 26, 2013 02:50

Hi Bruno,

Quote:

Originally Posted by wyldckat (Post 447953)
Greetings Stephen,

The internal ".foam" reader is allergic to the boundary condition "uniformFixedValue"...

So, this is a "real error", then, and not a red herring?

With that hack, the post-processing works; now I can tinker with the simulation to try and understand it.

Thanks for responding so quickly, you've always been an enormous help!

wouter September 12, 2013 11:31

Hello Wyldckat,
Do you have a trick like this for binary compressed files in paralel? I have this problem with paraview3.98.0
thanks
Wouter

wyldckat September 14, 2013 10:19

Greetings Wouter,

Quote:

Originally Posted by wouter (Post 451373)
Do you have a trick like this for binary compressed files in paralel?

Why yes, yes I do! :cool:
Although, the sed command should also work in binary and in parallel... something like:
Code:

sed -i -e "s=uniformFixedValue=fixedValue=g" processor*/[0-9][0-9]*/{U,p,k,nut,epsilon}
Anyway, the other trick is that OpenFOAM has a utility application called changeDictionary. It provides an example dictionary next to the source code: https://github.com/OpenFOAM/OpenFOAM...DictionaryDict

A quick summary "system/changeDictionaryDict" would be:
Code:

FoamFile
{
    version    2.0;
    format      ascii;
    class      dictionary;
    object      changeDictionaryDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dictionaryReplacement
{
    "(U|p|k|nut|epsilon)"
    {
        boundaryField
        {
            "(your|patch|names|here)"
            {
                type            fixedValue;
            }
        }
    }
}

Then use it by running the utility in parallel as well, the same way you ran the solver. For more information on options:
Code:

changeDictionary -help
Best regards,
Bruno


edit: Wouter found an issue with having to run changeDictionary for multiple times. A hack to do this is provided here: http://www.cfd-online.com/Forums/ope...tml#post452294 post #4


All times are GMT -4. The time now is 10:46.