CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM Paraview & paraFoam (
-   -   parallel case with paraview (

Ingenieur August 5, 2013 04:10

parallel case with paraview
Hi every one :)

I have a problem with paraview (parallel case):

I want to create an animation of parallzied case of 100 processors. I converted all timesteps to VTK files and I tried to add them to paraview but the problem is that I cann't create a common slice for the whole case (because the filters will be activated only for every processor alone)

do u have an idea to solve this problem?

I'll be grateful

thanks in advance


wyldckat August 16, 2013 08:07

Hi Mizo,

There are at least 3 possible ways for you to process this case:
  1. You first have reconstruct the results (using reconstructPar) and only then you can use foamToVTK.
  2. Or you have the case located in your local workstation and run:

    paraFoam -builtin
    Then choose in "Case Type" the option "Decomposed Case" and hit the "Apply" button. This way you can have the whole case open in ParaView, without the need for converting data.
  3. Or you can select all VTK "processor*" files in the "Pipeline Browser" and apply the filter "Group Datasets" and then work with the resulting group in the pipeline, instead of each individual VTK file.
Best regards,

Ingenieur August 16, 2013 08:24

Hi Bruno,

thanx for your reply. I reconstructed the whole timesteps for only two fields:

reconstructPar -fields "(U Cp)"

then I created an animation, It took a long time but it was the easiest way :)

many thanks again


All times are GMT -4. The time now is 00:10.