CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Visualization & Post-Processing Software > ParaView

[OpenFOAM] turbineSiting tutorial and paraview-3.98.0

Register Blogs Community New Posts Updated Threads Search

Like Tree2Likes
  • 1 Post By wyldckat
  • 1 Post By wyldckat

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 25, 2013, 14:20
Default turbineSiting tutorial and paraview-3.98.0
  #1
New Member
 
Stephen Bosch
Join Date: Feb 2013
Location: Germany
Posts: 22
Rep Power: 13
pajot is on a distinguished road
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.
pajot is offline   Reply With Quote

Old   August 25, 2013, 15:50
Default
  #2
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,982
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
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 likes this.
__________________
Last edited by wyldckat; August 25, 2013 at 15:50. Reason: see "edit:"
wyldckat is offline   Reply With Quote

Old   August 26, 2013, 03:50
Default
  #3
New Member
 
Stephen Bosch
Join Date: Feb 2013
Location: Germany
Posts: 22
Rep Power: 13
pajot is on a distinguished road
Hi Bruno,

Quote:
Originally Posted by wyldckat View Post
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!
pajot is offline   Reply With Quote

Old   September 12, 2013, 12:31
Default
  #4
Senior Member
 
Wouter van der Meer
Join Date: May 2009
Location: Elahuizen, Netherlands
Posts: 203
Rep Power: 18
wouter is on a distinguished road
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
wouter is offline   Reply With Quote

Old   September 14, 2013, 11:19
Default
  #5
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,982
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Greetings Wouter,

Quote:
Originally Posted by wouter View Post
Do you have a trick like this for binary compressed files in paralel?
Why yes, yes I do!
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
pajot likes this.
__________________
Last edited by wyldckat; September 17, 2013 at 19:41. Reason: see "edit:"
wyldckat is offline   Reply With Quote

Reply

« Previous Thread | Next Thread »

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 Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
[OpenFOAM] How to plot wall shear stress on T3A tutorial in paraview? ht2017 ParaView 1 February 19, 2018 19:01
Motobike tutorial U, P etc. data not loading to ParaView. Doug68 OpenFOAM Running, Solving & CFD 4 September 3, 2016 15:08
[OpenFOAM] Cavity Tutorial: ParaView starts, cannot find reader mfrain ParaView 7 June 18, 2012 23:14
Watching the chtMultiRegionFoam tutorial in Paraview anke OpenFOAM 1 March 1, 2010 09:38
[OpenFOAM] HI all I cant find display button in paraview when i execute cavity tutorial there is only parameter button in the paraview chan ParaView 2 February 13, 2006 08:37


All times are GMT -4. The time now is 10:52.

Contact Us - CFD Online - Privacy Statement - Top