CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Paraview & paraFoam

Paraview canot visualize codedFixedValue velocity

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 16, 2013, 15:08
Default Paraview canot visualize codedFixedValue velocity
  #1
Member
 
Ovie Doro
Join Date: Jul 2009
Posts: 99
Rep Power: 7
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, 13:08
Default
  #2
Member
 
Ken
Join Date: Aug 2012
Posts: 61
Blog Entries: 1
Rep Power: 4
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, 09:52
Default
  #3
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,251
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
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, 14:21
Default
  #4
Member
 
Ken
Join Date: Aug 2012
Posts: 61
Blog Entries: 1
Rep Power: 4
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, 14:37
Default
  #5
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,251
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
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
wyldckat is offline   Reply With Quote

Old   September 7, 2013, 14:50
Default
  #6
Member
 
Ken
Join Date: Aug 2012
Posts: 61
Blog Entries: 1
Rep Power: 4
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, 14:55
Default
  #7
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,251
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
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
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
WSS and normal velocity gradient for the slanted pipe wanna88 FLUENT 2 October 1, 2012 22:34
Problem with time average tangential velocity in swirl flow. lakhi FLUENT 5 July 18, 2012 16:28
paraFoam reader for OpenFOAM 1.6 smart OpenFOAM Installation 13 November 16, 2009 22:41
Velocity Under-relaxation in SIMPLE type methods Matt U. Main CFD Forum 6 July 4, 2005 05:29
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 09:11


All times are GMT -4. The time now is 18:22.