[openfoam_user]

Dear users,

1. How can I stop 'properly' a multi-processors job that is running in background ? and maybe also save the results of the last iterations ?

2. Is it possible to plot the residuals while the job is running ?

Thanks for helping me,

Stephane.

[gschaider]

Have a look at section 4.3 of the 1.5 UserGuide:

Replace in the controlDict the current stopAt-Value with writeNow. Save and wait. But be sure not to mistype because then your run might stop without writing anything

Bernhard

[openfoam_user]

Thanks Bernhard for your help !
Stephane.

[floooo]

During calculation you can make :

reconstructPar
paraFoam&

You can see the first output
and 20min later you can update it :

reconstructPar
in paraFoam => update content

in order to kill a job I use
ps to get the PID
kill ...

Then if you want to start from the last output, you have to modify your controlDict and change the start time.

[olesen]

For solvers that I use often, I've added the following bits of code.

1.
At the top bit of the main(), before the time loop starts:

// define ABORT file for stopping the job
fileName abortName(args.rootPath()/args.globalCaseName()/"ABORT");
if (file(abortName))
{
Info<< "removing old ABORT file" << endl;
rm(abortName);
}


2. In the bottom part of the time loop:

runTime.write();

Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s"
<< " ClockTime = " << runTime.elapsedClockTime() << " s"
<< nl << endl;

if (file(abortName))
{
Info<< "reacting to user ABORT" << endl;
runTime.writeAndEnd();
}


3. Finally outside of the time loop:


// cleanup ABORT file
if (file(abortName))
{
rm(abortName);
}



This makes the solver react to the existence of the file 'ABORT' and works well with serial or parallel calculations.

It could make a nice functionObject, but to be convenient there'd need to be some way of defining site or user global functionObjects. Eg, via the existing etc/controlDict mechanism, or with a ~OpenFOAM/... directory expansion.
I'd certainly want to avoid adding the functionObject to every single system/controlDict!

[openfoam_user]

Mark,

I am a new user of OpenFoam !!!

into which file (controlDict) have you written these bits of code ?

Stephane

[gschaider]

Hi Stephane!

Have a look at the chapter 4 of the user-guide. It is a most interesting read. Especially if you have to ask for the controlDict (which is THE most important file in any OF-case). Trust me.

Bernhard

[olesen]

The bits of code have been added directly into the solver itself (eg, simpleFoam, rhoSimpleFoam, rhoPorousSimpleFoam, etc.)