CFD Online Discussion Forums - [OpenFOAM] Paraview canot visualize codedFixedValue velocity

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- ParaView (https://www.cfd-online.com/Forums/paraview/)

- - [OpenFOAM] Paraview canot visualize codedFixedValue velocity (https://www.cfd-online.com/Forums/paraview/122315-paraview-canot-visualize-codedfixedvalue-velocity.html)

Paraview canot visualize codedFixedValue velocity

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.

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?

Greetings to all!

A few questions

Which ParaView version you're using?
Which OpenFOAM version you're using?
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.
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

Quote:

Originally Posted by wyldckat (Post 450387)

Greetings to all!

A few questions

Which ParaView version you're using?
Which OpenFOAM version you're using?
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.
Can you reproduce the same issue with a tutorial in OpenFOAM or can you provide an example case?

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!

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

Good to know.

If I instead launch Paraview using 'paraFoam', should it work? I am connecting remotely (pvserver).

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