[balkrishna]

Hi ,

How do i name blocks in a blockMeshDict file ? For example ,
a line of my blockMesh reads as follows :

blocks
(
hex (0 1 2 3 12 13 14 15) (20 1 20) simpleGrading (1 1 1)
...
)

How do i give it a name ? Something like "Region 1" ?
Also how do i output the average of this region at every timestep ?

Thanks .

[MartinB]

For the first question: you can do it like this:

hex (0 1 2 3 12 13 14 15) Region_1 (20 1 20) simpleGrading (1 1 1)

Martin

[balkrishna]

Thanks ... How do i output the average of some value , say: gas holdup ,in this region at every timestep ?

[gschaider]

Originally Posted by balkrishna

Thanks ... How do i output the average of some value , say: gas holdup ,in this region at every timestep ?

I'm not aware of a way to do this with "standard"-OpenFOAM. I like to do that kind of calculation with swak4Foam (but I'm a bit biased in that respect)

[Bernhard]

Originally Posted by balkrishna

Thanks ... How do i output the average of some value , say: gas holdup ,in this region at every timestep ?

I think there is a volume average that you can use in the functions subdictionary using the sampling library, or, if you want to calculate it afterwards, you can probably just use the sample utility.

[balkrishna]

I figured out a way to do the same . The code for the same is as follows :

{
    const scalarField& V = mesh.V();

    forAll(mesh.cellZones(), czi)
    {
        const labelList& cellLabels = mesh.cellZones()[czi];
        //      const volScalarField& alpha = phasea.alpha() ; 
        
        scalar phaseVolume = 0;
        scalar zoneVol = 0;
        forAll(cellLabels, cli)
          {
            label celli = cellLabels[cli];
            phaseVolume += alpha[celli]*V[celli];
            zoneVol += V[celli] ;
          }
        
        reduce(phaseVolume, sumOp<scalar>());

        Info<< " phase volume in zone " << mesh.cellZones()[czi].name() << " of volume  " << zoneVol << " " <<phaseVolume << endl ;
            
        
    }
}

This works perfectly fine in serial runs , however in parallel runs it gives absurd answers . For eg : in parallel runs it outputs the value of the zoneVol (the volume of the zone ) as 0 while in the serial runs it outputs the correct volume values .

Can anyone help me out with this ?

[MartinB]

Hi,

you must use the reduce command for the zoneVol, too:

               ...
               zoneVol += V[celli] ;
          }
        reduce(zoneVol, sumOp<scalar>()); // <--------
        reduce(phaseVolume, sumOp<scalar>());

Martin

[balkrishna]

Thanks a lot .....