[KarenRei]

I've got a simulation that's running abnormally slow in order to try to prevent exceeding its specified maximum courant number. Looking at the data in paraview, nothing appears out of the ordinary. So the idea obviously came to mind to plot the courant number itself in paraview / parafoam. However, "postProcess -func CourantNo" is giving up:

--> FOAM FATAL ERROR: 

    request for volScalarField rho from objectRegistry region0 failed
    available objects of type volScalarField are
1(surfaceSum(mag(phi)))

    From function const Type& Foam::objectRegistry::lookupObject(const Foam::word&, bool) const [with Type = Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>]
    in file /opt/OpenFOAM-v1806/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 239.

Thoughts?

[piu58]

It is much easier to send the log file through a grep or awk script which gives the Courant number together with some other data like simulated time.

[RobertHB]

OpenFoam also offers a Courant Number function which you can add to your controlDict.

functions
{
#includeFunc CourantNo
 }

Source.
And then you could use the foam monitor to plot the Co number if i'm not mistaken.

[KarenRei]

Originally Posted by piu58

It is much easier to send the log file through a grep or awk script which gives the Courant number together with some other data like simulated time.

That would give the max and average courant number, but not show where the number is high.

[KarenRei]

Originally Posted by RobertHB

OpenFoam also offers a Courant Number function which you can add to your controlDict.

functions
{
#includeFunc CourantNo
 }

Source.
And then you could use the foam monitor to plot the Co number if i'm not mistaken.

How would foamMonitor show me in what cells the courant number is high?

[RobertHB]

It doesn't, i misunderstood your endavour. You can always calculate your Co. in paraview with the calculator. But it will be an mirrorimage of your velocity.

[KarenRei]

It's more than just velocity, the cell size with respect to the velocity vector matters. It's not enough just to display U in paraview.

[miotto]

Originally Posted by KarenRei

I've got a simulation that's running abnormally slow in order to try to prevent exceeding its specified maximum courant number. Looking at the data in paraview, nothing appears out of the ordinary. So the idea obviously came to mind to plot the courant number itself in paraview / parafoam.

So here is how you do it:


First, you add the Courant number function object to your ControlDict:

functions
{
    Co1
    {
        type                CourantNo;
        libs                ("libfieldFunctionObjects.so");
        executeControl      timeStep;
        executeInterval     2;
        writeControl        writeTime;
    }
}

Run you simulation and open paraView. There you have to add the VolumeField Co by checking the "Co" checkbox under Properties/Volume Fields and clicking on apply.



Then advance to the second timestep of you simulation and the Co will be available for visualization (as the other regular variables - pressure, velocity, etc.)