[AqeelAhmed168]

Paraview can be used to visualize a decomposed case (without reconstruction) with the original parallel format of OpenFoam (a seperate directory for each processor).
Since version 5, there is a new collated format for parallel decomposition (one directory irrespestive of the number of domains).

Is it possible to visualise the same without reconstructing the case?

[Michael@UW]

Originally Posted by AqeelAhmed168

Paraview can be used to visualize a decomposed case (without reconstruction) with the original parallel format of OpenFoam (a seperate directory for each processor).
Since version 5, there is a new collated format for parallel decomposition (one directory irrespestive of the number of domains).

Is it possible to visualise the same without reconstructing the case?

Hi AqeelAhmed168,

Do you know how open the collated parallel files in paraview? I use mpirun -np 16 foamFormatConvert -fileHandler allocated -parallel to convert the results; then processor1-15 are deleted and processors16 is remained. But I do not know how to load them into paraview.
I created a dummy file case.foam in processors16 then 'paraview case.foam' but there is an error showing something like "processors16/constant/polyMesh/boundary: Expected keyword, closing brace, ';' or EOF, found ". No data is shown in paraview but the total time steps are shown correctly in "Current Time Control" (toolbar).

By the way, I use openfoam7 and the shipped paraview was not compiled but an official paraview 5.8 was installed separately.

I am not sure if paraFoam must be used to load the new collated file format. Hope someone can give me a hint.

Thanks,
Michael

[reza_azadi]

Hi. Could any body let me know how can I open "collated" format of openfoam files as decomposed in ParaView? I created a dummy file with .foam extension, at it does not read in anything to ParaView.

[jherb]

Currently, the collated format is not supported by the OpenFOAM reader in paraview. There are bug reports/merge requests to add supported, but it looks like, the work has stalled:
https://gitlab.kitware.com/vtk/vtk/-/issues/17096
https://gitlab.kitware.com/vtk/vtk/-..._requests/4003

[reza_azadi]

Originally Posted by jherb

Currently, the collated format is not supported by the OpenFOAM reader in paraview. There are bug reports/merge requests to add supported, but it looks like, the work has stalled:
https://gitlab.kitware.com/vtk/vtk/-/issues/17096
https://gitlab.kitware.com/vtk/vtk/-..._requests/4003

Thanks for the reply! So, it seems the only option for me is to convert the data to uncollated format. I tried to do so using foamFormatConvert, but it only converts the mesh and there is no information about the fields in the processor folders. Do you have any idea what is happening? I use OpenFOAM V1906 and mesh is refined each 10 time steps, giving different mesh domains for the saved times.

For the record, I use the following command to uncollate the data. based on what https://www.openfoam.com/releases/op...2/parallel.php suggests:

mpirun -np 4 foamFormatConvert -fileHandler uncollated -parallel

[jherb]

I just use reconstructPar.

[reza_azadi]

Originally Posted by jherb

I just use reconstructPar.

The problem with reconstructPar (& reconstructParMesh) is that the result is a whole file for each time step, and I cannot post-process the data in parallel in ParaView. My cases are large (~12 million mesh grids) and processing them in serial is not feasible for me. It takes ~4h to see the result of an applied filter. D3 filter can distribute the data into cores and make it parallel-aware, but I think it works only for unstructured mesh, which is not the case for me.

[reza_azadi]

Originally Posted by reza_azadi

The problem with reconstructPar (& reconstructParMesh) is that the result is a whole file for each time step, and I cannot post-process the data in parallel in ParaView. My cases are large (~12 million mesh grids) and processing them in serial is not feasible for me. It takes ~4h to see the result of an applied filter. D3 filter can distribute the data into cores and make it parallel-aware, but I think it works only for unstructured mesh, which is not the case for me.

Following this question, I contacted Dr. Yeon, who initiated the discussion on collated format support with ParaView team 3 years ago. Here is a short part of his answer to my question:

"...To make story short, the OpenFOAM reader implemented in ParaView needed redesign for better design to adopt collated format.

So, ParaView/VTK team were discussing about redesign of the reader but any news is not on the list yet.

After that point, I did not pay attention to the reader implementation. instead I just was using uncollated format..."

So, for the ones with the same concern, there are two possible solutions for this issue right now: 1) Convert the data into uncollated format, 2) reconstruct the data into one.

[Michael@UW]

Hi Reza,
Thanks for your infomation!
It seems collated is not mush useful unless we can post-process collated data.

[reza_azadi]

Originally Posted by Michael@UW

Hi Reza,
Thanks for your infomation!
It seems collated is not mush useful unless we can post-process collated data.

Hi Michael,

I would say it depends. For example, my case requires using dynamic mesh, which generates different mesh domains at different type steps. I do not why, but when I use uncollated format, the simulation crashes after hundreds of time steps and gives an error of not being able to create the polymesh folder in a folder corresponded to one of the processors and fails to write the data. This happens randomly. I did not have a similar issue for collated format, at all. So, I ran my cases in collated format and now I am trying to use foamFormatConvert to convert the format back into uncollated, using which I can post-process the data in parallel in ParaView.

[Michael@UW]

It' weired you can run the simulation using collated format but un-collated.

The collated format is designed to handle the limitation of the total files that can be created in a folder. The only potential usage I think of is the following case. You have a computer that can only create, say, 1M files. So you run the simulation on it with the collated format. After the simulation, you copy the files to another computer which does not have this limitation and convert them back to un-colloated type. But it makes no sense if the simulation and post-processing are conducted on the same computer. Or it runs faster if using collated format?