Problem with "cloud - lagrangian" - it is missing from the Mesh part

I downloaded ParaView 5.11.0 version and tried to visualize a case from OpenFoam 10 (*.foam file) that includes particles. I know that I should check “cloud - lagrangian” from the Mesh Regions, and to do “Extract block” after that, but the problem is that there is no such option to check in the Mesh parts - there is no “cloud - lagrangian”. I am not at the zero time, so the particles should present in the mesh. What should I do to be able to visualize the particles?
Thank you in advance!
Best Regards!

Hi and welcome @ni8 !

Please share your dataset.


Hi, Mathieu!
Thank you for your reply!

Here is my dataset: WeTransfer - Send Large Files & Share Photos Online - Up to 2GB Free

Thank you for your time!
Best regards!

There is indeed no such mesh regions, why do you expect such region to be present ?


Hi, Mathieu!
When this case is visualized through OpenFoam (typing paraFoam in the terminal), there is such mesh region in the Mesh part of the ParaView window, which I can check and the particles are then visualized.

But when I try to visualize them in the downloaded version of ParaView, there is no such mesh region. I am new in this and I thought that maybe there is something that I missed like some plugin for example…

Could you please recommend how could I add such mesh region, because I see that the particles are added in the simulation (in the log file during the simulation) and also in the results there is folder “lagrangian”, in which there is data for the cloud.

Sorry if my question is stupid, but as I mentioned I am new in this. :slight_smile:

Best regards!

paraFOAM provide a plugin with a completely different code than the OpenFOAM reader in ParaView.

Maybe this is a missing feature in ParaView, you can read this:

Thank you very much for your answer, Mathieu!

I guess that these paraFoam script/modules cannot be added to the ParaView that I have and I should look for another solution of the problem, right?

Best regards!

It sounds like your are using the .org flavour (from the OpenFOAM Foundation Ltd) instead of the .com flavour (from OpenCFD Ltd.). In the .com version, the cloud coordinates as “positions” (containing x,y,z, celli,…) and “coordinates” (containing the barycentric coordinates). In the .org version, they decided to write a “positions” file that contains the barycentric coordinates. The ParaView/VTK reader can handle a “positions” file containing x,y,z,… but not the barycentric version, since this would entail creating the entire volume mesh and calculating the barycentric coordinate mapping in order to obtain the x,y,z positions to display the cloud. This is a crazy amount of work and a maintenance nightmare, which is why you might consider alternatives such as a coordinates to positions conversion utility (saw something posted on cfd-online), foamToEnsight or foamToVTK converting the clouds only, or use the .com version.


Adding the OpenFOAM reader modules into ParaView/VTK is definitely a non-starter. It is completely differently structured, non-parallel, would require almost all of OpenFOAM as a build dependency for VTK etc.

1 Like

Dear Mark,
Sorry for my so late response!

I just wanted to thank you very much for these detailed explanations! I use exactly the .org version as you said. I will try coordinates to positions conversion as you suggested.

Best Regards!