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

[OpenFOAM] Paraview canot visualize codedFixedValue velocity

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

Like Tree1Likes
  • 1 Post By wyldckat

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 16, 2013, 16:08
Default Paraview canot visualize codedFixedValue velocity
  #1
Member
 
Ovie Doro
Join Date: Jul 2009
Posts: 99
Rep Power: 16
ovie is on a distinguished road
Hi Foamers:

I have a codedFixedValue boundary condition (for velocity and wall motion) at a moving wall boundary. But when I load up the case on paraview, it gives an error when trying to read the velocity and pointsMotion files. Error message looks like:

" Error reading line xxx of casename/0/U: Unsupported directive { "

As a result I canot load velocity files and cant generate streamlines for the simulation.

Is there a way around this??

Thanks.
ovie is offline   Reply With Quote

Old   September 2, 2013, 14:08
Default
  #2
Member
 
Join Date: Aug 2012
Posts: 68
Blog Entries: 1
Rep Power: 13
Nucleophobe is on a distinguished road
I have the same problem. Did you find a solution?

Edit:
You *can* delete the code block ('#{' to '#}') out of the appropriate results files, but this is a bit painful. I'm not sure what effect it has on subsequent time steps either.

Is there another way to make paraview cooperate?
Nucleophobe is offline   Reply With Quote

Old   September 7, 2013, 10:52
Default
  #3
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,974
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 to all!

A few questions
  1. Which ParaView version you're using?
  2. Which OpenFOAM version you're using?
  3. Which file extension you are using, namely if it is ".OpenFOAM" or ".foam"?
    • More specifically, if you are using OpenFOAM's reader for ParaView or the internal reader, respectively.
  4. Can you reproduce the same issue with a tutorial in OpenFOAM or can you provide an example case?
I ask all of this because I've used OpenFOAM 2.2.x, ParaView 3.12.0, OpenFOAM's reader for ParaView, by simply running paraFoam in the tutorial "incompressible/simpleFoam/pipeCyclic" and I had absolutely no problem!
And this tutorial uses code for "0/U".

Best regards,
Bruno
__________________
wyldckat is offline   Reply With Quote

Old   September 7, 2013, 15:21
Default
  #4
Member
 
Join Date: Aug 2012
Posts: 68
Blog Entries: 1
Rep Power: 13
Nucleophobe is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
Greetings to all!

A few questions
  1. Which ParaView version you're using?
  2. Which OpenFOAM version you're using?
  3. Which file extension you are using, namely if it is ".OpenFOAM" or ".foam"?
    • More specifically, if you are using OpenFOAM's reader for ParaView or the internal reader, respectively.
  4. Can you reproduce the same issue with a tutorial in OpenFOAM or can you provide an example case?
I ask all of this because I've used OpenFOAM 2.2.x, ParaView 3.12.0, OpenFOAM's reader for ParaView, by simply running paraFoam in the tutorial "incompressible/simpleFoam/pipeCyclic" and I had absolutely no problem!
And this tutorial uses code for "0/U".

Best regards,
Bruno
1) Paraview 4.0.1
2) OpenFOAM 2.1.x
3) case.foam file, opened from Paraview (not paraFoam)
4) I actually get the error:
Code:
Making dependency list for source file codeStreamTemplate.C
codeStreamTemplate.C(61): error: invalid line number
          #line 0 ""
                ^
when running blockMesh in "incompressible/simpleFoam/pipeCyclic", but this is probably unrelated. The codedFixedValue code works fine in the case I am using.

Thanks Bruno!
Nucleophobe is offline   Reply With Quote

Old   September 7, 2013, 15:37
Default
  #5
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,974
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
Hi Ken,

Unfortunately the internal reader in ParaView 3.12.0 to 4.0.1 cannot handle many of the new things that have been implemented since OpenFOAM 2.0.0.

The only fail-safe measure I can suggest is to rely on foamToVTK:
Code:
foamToVTK -poly
The option is explained by the option "-help"

Then open in ParaView the files that are in the newly created VTK folder.

The other possible solution (that I haven't tested) is to build the latest plug-in that Takuya has made: http://openfoamwiki.net/index.php/Co...r_for_ParaView
But this requires that you also build ParaView from source code...

Best regards,
Bruno
josephchou likes this.
__________________
wyldckat is offline   Reply With Quote

Old   September 7, 2013, 15:50
Default
  #6
Member
 
Join Date: Aug 2012
Posts: 68
Blog Entries: 1
Rep Power: 13
Nucleophobe is on a distinguished road
Good to know.

If I instead launch Paraview using 'paraFoam', should it work? I am connecting remotely (pvserver).
Nucleophobe is offline   Reply With Quote

Old   September 7, 2013, 15:55
Default
  #7
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,974
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
If the paraFoam command is opening with the file extension ".OpenFOAM" and is using OpenFOAM's own plug-in reader, then it should work. Although it won't be able to load decomposed cases.

If by any chance you want to build OpenFOAM's own plug-in for ParaView 4.0.1, see this bug report: http://www.openfoam.org/mantisbt/view.php?id=621
__________________
wyldckat is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
UDF comilation error. urgent help please m zubair Fluent UDF and Scheme Programming 4 February 10, 2019 12:19
visualize the particle with various diameter using Paraview openfoammaofnepo OpenFOAM 3 June 25, 2018 18:18
Setting velocity profile at the inlet using codedFixedValue CTR OpenFOAM Pre-Processing 1 May 20, 2014 13:01
[OpenFOAM] Visualize pointSet in ParaView Arnoldinho ParaView 2 July 12, 2012 05:58
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 10:11


All times are GMT -4. The time now is 05:38.