[scfd]

Hi,

I need to calculate average velocity components and temperature of a specified volume in a container at every time-step. It is the same thing that averaging specific volume fraction inside a pipe. I couldn't find which utilites I should use.

• How can I define a custom volume inside the container? (setSet, topoSet?)
• How can I calculate the average of this volume in each time step? (volFieldValue?)

regards,
scfd.

[Yann]

Hello scfd,

You seem to already have the answers to your questions!

You can indeed use volFieldValue to compute average values in a volume.
Your volume can be a cellZone, and you can create this cellZone right from snappyHexMesh when meshing (assuming you are meshing with snappy) or on an existing mesh using topoSet.

In topoSet you can use a source such as boxToCell or cylinderToCell to select the cells inside the volume you want to average. This will create a cellSet, then you can use setToCellZone to convert your cellSet into a cellZone.

Regards,
Yann

[scfd]

Originally Posted by Yann

Hello scfd,

You seem to already have the answers to your questions!

You can indeed use volFieldValue to compute average values in a volume.
Your volume can be a cellZone, and you can create this cellZone right from snappyHexMesh when meshing (assuming you are meshing with snappy) or on an existing mesh using topoSet.

In topoSet you can use a source such as boxToCell or cylinderToCell to select the cells inside the volume you want to average. This will create a cellSet, then you can use setToCellZone to convert your cellSet into a cellZone.

Regards,
Yann

Dear Yann,

Thanks for your quick reply. I followed your suggestion and nearly reach what I want. Here is the topoSet file and fucntion:

actions
(
    {
        name        packVolume;
        type        cellSet;
        action      new;
        source      cylinderToCell;
        point1      (0 0 30);
        point2      (0 0 70);
        radius      30;
    }
    {
        name    volpack;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        set     packVolume;
    }
);

functions
{   

	vfv1
	{
		type            volFieldValue;
		libs            (fieldFunctionObjects);
		fields          (T U);
		operation       average;
		regionType     cellZone;
		name            volpack;
		writeFields     true;
		writeToFile     true;
		writeControl    writeTime;
	}
}

Case running smoothly but I get the following line and vfv1 returns empty output:

--> FOAM Warning : 
cellZone(volpack):
    Region has no cells


    From void Foam::functionObjects::volRegion::calculateCache()
    in file functionObjects/volRegion/volRegion.C at line 122.
--> loading function object 'vfv1'

Where could I have made a mistake?

regards,
scfd.

[Yann]

Looks like volPak is empty, what is the output when executing topoSet?

Regards,
Yann

[scfd]

Originally Posted by Yann

Looks like volPak is empty, what is the output when executing topoSet?

Regards,
Yann

Here:

Reading topoSetDict

Time = 0
    mesh not changed.
Created cellSet packVolume
    Applying source cylinderToCell
    Adding cells with centres within cylinder, with point1 = (0 0 30), point2 = (0 0 70), radius = 30
    cellSet packVolume now size 22935
Created cellZoneSet volpack
    Applying source setToCellZone
    Adding all cells from cellSet packVolume ...
    cellZoneSet volpack now size 22935

End

regards,
scfd

[Yann]

This is uncanny, since your cellZone seems to be properly created during topoSet.
Just a question: do you run your case in parallel? If you do, have you run topoSet in parallel too?

Regards,
Yann

[scfd]

Originally Posted by Yann

This is uncanny, since your cellZone seems to be properly created during topoSet.
Just a question: do you run your case in parallel? If you do, have you run topoSet in parallel too?

Regards,
Yann

Dear Yann,

This is the workflow:

runApplication blockMesh
runApplication snappyHexMesh -overwrite
runApplication topoSet
runApplication checkMesh 
transformPoints -scale "(0.001)"
runApplication createPatch -overwrite
runApplication renumberMesh -overwrite
restore0Dir
runApplication changeDictionary
runApplication decomposePar
#runParallel $(getApplication)
#runApplication reconstructPar

checkMesh detect the cellZone:

Checking basic cellZone addressing...
                CellZone        Cells       Points       VolumeBoundingBox
                 square        21285        28654     92044.29 (-16.240871 -16.24087 0) (16.24087 16.240869 100)
            innerCircle        21000        24480     195490.6 (-30.458205 -30.458205 0) (30.458204 30.458205 100)
                volpack        22935        29794    112415.39 (-30.458205 -30.458205 30.005496) (30.458204 30.458205 69.994475)

But some strange things happens when I run createPatch:

--> FOAM Warning : 
    From void Foam::polyTopoChange::addMesh(const Foam::polyMesh&, const labelUList&, const labelUList&, const labelUList&, const labelUList&)
    in file polyTopoChange/polyTopoChange.C at line 2346
    Cell:42283 centre:(-0.0055351021 0.0060833295 0.056633843) is in two zones:square and volpack
    This is not supported. Continuing with first zone only.
--> FOAM Warning : 
    From void Foam::polyTopoChange::addMesh(const Foam::polyMesh&, const labelUList&, const labelUList&, const labelUList&, const labelUList&)
    in file polyTopoChange/polyTopoChange.C at line 2346
    Cell:42284 centre:(-0.0060848722 0.0060845366 0.056656412) is in two zones:square and volpack
    This is not supported. Continuing with first zone only.
Moving faces from patch z_min_0 to patch 4
Moving faces from patch z_max_0 to patch 5
Moving faces from patch wall_0 to patch 6
Moving faces from patch STL_spheres_0 to patch 7
Doing topology modification to order faces.
Not synchronising points.
Removing patches with no faces in them.
Removed zero-sized patch wall_0 type wall at position 0
Removed zero-sized patch z_min_0 type wall at position 1
Removed zero-sized patch z_max_0 type wall at position 2
Removed zero-sized patch STL_spheres_0 type wall at position 3

Writing repatched mesh region0 to 0

End

Maybe this step is the problem.

regards,
scfd

[Yann]

I'm not sure why createPatch would mess with the cellZone, but you can try to run topoSet after createPatch or even right before running decomposePar, just to be sure there is nothing else messing with the cellZone definition.
(And if it still doesn't solve the issue, you can ultimately run it after decomposing the case with runParallel topoSet)

Yann

[scfd]

Originally Posted by Yann

I'm not sure why createPatch would mess with the cellZone, but you can try to run topoSet after createPatch or even right before running decomposePar, just to be sure there is nothing else messing with the cellZone definition.
(And if it still doesn't solve the issue, you can ultimately run it after decomposing the case with runParallel topoSet)

Yann

...right before running decomposePar

That solved the problem. Many thanks Yann.

runApplication blockMesh
runApplication snappyHexMesh -overwrite
runApplication checkMesh 
runApplication transformPoints -scale "(0.001)"
runApplication createPatch -overwrite
runApplication renumberMesh -overwrite
restore0Dir
runApplication changeDictionary
runApplication topoSet
runApplication decomposePar
runParallel $(getApplication)
runApplication reconstructPar

regards,
scfd