CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM Paraview & paraFoam (
-   -   How to run paraFoam parallel? (

sandy March 13, 2012 08:38

How to run paraFoam parallel?
Hi friends, there are six cores in my computer workstation? Can I also run paraFoam parallel? Who know how to do? Thank you very much.

MartinB March 13, 2012 10:13

Hi Sandy,

it will not make much sense to run ParaView in parallel on your workstation. The graphic card will do the rendering much faster than your 6 cores can do, and to speed up the pure data management it's more important to have fast hard disc drives.

If you still want to run ParaView in parallel you must compile it with some flags enabled: edit the makeParaView script in the ThirdParty directory and enable "withMPI=true" (path to mpi.h might be necessary to be added). You can enable "withMESA", too, so the rendering is done with your CPU instead of the graphic card.

You then have to start the ParaView server application (pvserver) and log in with a ParaView client.

The pvserver will run in busy waiting mode by OpenMPI's default, which will slow down your system's performance for other tasks. You must compile MPI on your own to avoid this behaviour.

A situation where it makes sense to use ParaView in parallel is: you have a remote cluster with plenty of hard discs and multiple nodes, your mesh is really large (let's say 100.000.000 cells, so it does not fit into your local machine's memory) and it's properly distributed over all the servers hard discs. You are sitting at your notebook and start the ParaView server application on the cluster. You log in to the ParaView server, which does the data management and rendering, and you receive the readily rendered screen output on your notebook.

Hints to speed up ParaView on your 6 core workstation:
- use binary format for your result files (can be set in the controlDict)
- import only the stuff you need (only U, if you want to make an animation using it, but not p or rho and other stuff, which is not shown at the current ParaView session)
- use static mesh caching in ParaView
- use "Ignore Time" option for the pipelines that do not change from time step to time step
- use ParaView's native OpenFOAM reader in the parallel mode (Decomposed Case), and distribute the processor* directories on different hard discs (using symbolic links)

Good luck


Dan N March 3, 2014 19:28

Stream Tracer calculation in ParaView
Hey MartinB

I am very new to OpenFoam and to CFD-Online so perhaps this is a trivial question.

I am looking at stream tracers to obtain the reattachment point of a boundary layer, and I must say that it is not running smooth.

In the post to Sandy you say that the graphic card will do the rendering much faster. My questions is: Is it my GPU or CPU that dose the Stream Tracer calculation ? or is it a combined effort ?

I guess that from the fact that U is a double number from C it might need to be the CPU.

PS. I am running a SSD so the speed of the hard drive is not the problem and 2x5850 AMD GPU so that shut be OK as well. And I will try you hints for speeding up the ParaView


MartinB March 4, 2014 04:57

Hi Dan,

I think, the CPU is the limiting factor for your stream tracer visualization.
You can try to rotate the finished stream lines with your left mouse button pressed, if this is smooth (with Settings->Render View->LOD Threshold = Off), than the GPU has no problem. If the rotation is not smooth, than you might need to install the proprietary video drivers from AMD.

Something costly for the GPU is the volume rendering of a scalar value.


All times are GMT -4. The time now is 06:47.