Running Paraview parallel
 

Hi all,

i am using paraview for 2 years now and I wanna use my 6 cores for the rendering now. For that I have to compile ParaView like the introduction given here:

http://paraview.org/Wiki/ParaView:Build_And_Install

I installed all Prerequisites but when i wanna configure my paraview settings with ccmake and switch on "use MPI" and set the MPI_LIBRARY path I ll get these messages:

I installed openMPI with
[code]
./configure --prefix=/home/shorty/OpenFOAM/openMPI
make
make install
[/make]

After that I get the libs in that folder under "libs/" there is for example the file libmpi.so ect...

well I do not understand why I can t fix that problem!
Do someone know that problem? Or I am doing sth. wrong?

Thanks in advance
Tobi

Hi Tobi,

I haven't been doing any big builds of ParaView lately, but I've written a lot on this subject, which is mostly accessible from here: Related issues to ParaView with OpenFOAM - Fixes and solutions

You'll find instructions on how to get ParaView 3.12.0 with everything on it for OpenFOAM consumption here: ParaView 3.12.0 SuperBuild on OpenFOAM - Well, not everything on it, but all of the default stuff that is officially installed in the builds provided at http://www.paraview.org

Additionally, on that blog post about the SuperBuild, it should be possible to use 3.14.1 instead of 3.12.0; for the modified source code for 3.14.1, visit this project: https://code.google.com/p/unofficial...ew-dev-install - but remember: you should still use the folder name for 3.12.0 on disk, just so you don't need to change anything on OpenFOAM settings files ;)

Best regards,
Bruno

Hi Bruno,

its only you who is answering me :)
Thanks for that - all the time!

Okay I tryed it with PV3.12 but with the same result.
Build openmpi again into

$HOME/OpenFOAM/openMPI/

-> there are include and lib folders and the files are in it.
Set the path in ccmake to /home/shorty/OpenFOAM/openMPI
/home/shorty/OpenFOAM/openMPI/lib
/home/shorty/OpenFOAM/openMPI/lib/
/home/shorty/OpenFOAM/openMPI/lib/libmpi.so
.
.
.

but without succsess

While compiling openmpi i get those warnings (maybe thats the problem?)

I ll have a look at your links tomorrow - i am too tierd now!

Wow Bruno, thats the truth! THANKS TO YOU - ALL THE TIMES!


Tobi

Have you found a solution?



To use paraview in parallel (e.g. 4 cores) I open a shell and type:


mpirun -np 4 pvserver


Afterwards I start paraview. I click on "connect" and then on "add server". Adjust the name and go to configure where I choose Startup Type "manual". Then I save it. Now I can choose the server in the list and click on apply.


If you now go to View and click on Memory inspector you can see that you are connected to the pvserver which uses 4 cores.


It is well document in the paraviewusersguide in chapter fiften: REMOTE AND PARALLEL VISUALIZATION

Hi Lukas,

As far my understanding is concerned you are mentioning about remote computers. Can you please let me know how to use the available cores on my local computer to run paraview in parallel. I have a 7 million cell data and Q-criteria is consuming almost half a day to get displayed. It would be great if you can give some insight. I have a 4 core workstation, with 32 gb ram and 1 gb graphics.

Thank you.

I am mentioning a local computer with e.g. 4 processors. Try the instructions I gave and / or read the Paraview user guide's section. It is working.


With respect to the Q-criteria you should maybe try not to display it in the whole CFD domain. Try a contour-filter with a specific value for the Q-criteria or a threshold filter with a SMALL range of values. This will be much less computational expensive. If you do not see anything decrease/ increase the value by a factor of 10 until you see something.

Hi Lukas,


I'm trying to run Paraview in parallel mode inside Ubuntu desktop 18 with 4 cores. When I execute mpirun -np 4 pvserver I have the following:


Waiting for client...
Connection URL: cs://4PI:11111
Accepting connection(s): 4PI:11111
Waiting for client...
Connection URL: cs://4PI:11111
ERROR: In /home/buildslave/dashboards/buildbot/paraview-pvbinsdash-linux-shared-release_superbuild/build/superbuild/paraview/src/VTK/Common/System/vtkSocket.cxx, line 206
vtkServerSocket (0xc24de0): Socket error in call to bind. Address already in use.



I dont have the firewall on.


Does anyone know how I can solve this problem? Thanks.






Edit: solved!

How did you solve it?

Instead of using the mpirun command, I install Paraview from the official page and I use the executable mpiexec from the /bin directory of Paraview: mpiexec -np cores pvserver

Maybe it's because the precompiled version of Ubuntu does not have mpi enabled. I do not know exactly.

Hi all ..
I would ask you where is written the server name ?

I wanted to keep the files on the Cluster and visualize the results on my local computer. Moreover, I wanted to run ParaView (PV) in parallel on the cluster.

Make sure to install the same PV versions on the cluster and local machine.

Using Linux systems I did this:

terminal 1:

change dir to paraview/bin directory and execute for 4 cores in parallel:
./mpiexec -np 4 ./pvserver --force-offscreen-rendering --server-port=11111
here I needed to use the mpiexec command instead of the mpi command, suggested by my solution.


terminal 2:

ssh -L '11111:node131.cluster:11111' -N yourUserNameOnCluster@yourClusterIP


Note: Nothing is happening in the termal but the command is working. Morever, I do not know why I have to do this.


terminal 3:

connect to server via GUI on local machine (Server Type: Client/Server; Host: localhost; Port: 11111)