[Daniel_C]

Since OpenFOAM V8 it should be possible to have the field values processed on a faceZone.

If I add a function file in the system directory in this way e.g. :

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  9
     \\/     M anipulation  |
-------------------------------------------------------------------------------
Description
    Calculates the average values of fields on a faceZone.

\*---------------------------------------------------------------------------*/

        type            surfaceFieldValue;
        libs            ("libfieldFunctionObjects.so");
        writeControl    timeStep;
        writeInterval   1;
        log             yes;
        writeTotalArea  no;
        writeFields     no;
        regionType      faceZone;
        name            my_facezone;
        operation       areaAverage;
	fields  
	(
	    U
	);

// ************************************************************************* //

and additionally include the function in controlDict via "#includeFunc my_function" entry, OpenFoam V9 throws an exception during solver initialization:

surfaceFieldValue my_function: faceZone(my_facezone):
Unable to process internal faces for volume field U

The same is true for other scalars (p for example), except for phi. When taking phi as a field variable, everything is fine. Also, the function faceZoneFlowRate works with phi.

Seems there is something I missed? Can anyone give me a hint, what I am doing wrong?

Regards

Daniel

[tomf]

Hi Daniel,

I once had a similar issue:

This is caused by the fact that the field values (U, p, etc.) are stored on the cell center. phi however is stored at the faces as it is the flux through the face.

You can use another functionObject first to interpolate the fields to the faces and afterwards you can use the surfaceFieldValue functionObject.

Have a look at the online documentation.

Hope it helps.
Cheers,
Tom

[Daniel_C]

Thank you Tom!

That worked for the field U in that way:

1. added the function my_surfaceInterpolate to interpolate field U to surface field UInterp

2. defined faceZoneAverage inline with name of faceZone und newly created field UInterp

That works for p in the same fashion. Great so far!

functions
{
    my_surfaceInterpolate
    {
     type        surfaceInterpolate;
     libs        ("libfieldFunctionObjects.so");
     fields      ((U UInterp)); 
     executeControl  timeStep;
     writeControl    writeTime;   
    }

    #includeFunc faceZoneAverage(name=my_faceZone, UInterp)

}

But, this doesn't work with the magnitude of U, because it calculates a constant average magnitude of 0 m/s for all time steps. It should not be zero, because there is definitely air flowing through the faceZone.

Here is what I have done:

    #includeFunc  mag(U)

    surfaceInterpolate1
    {
     type        surfaceInterpolate;
     libs        ("libfieldFunctionObjects.so");
     fields      ((mag(U) magUInterp)); 
     executeControl  timeStep;
     writeControl    writeTime;   
    }

    #includeFunc faceZoneAverage(name=my_faceZone, magUInterp)

Any ideas?


Regards

Daniel

[Daniel_C]

My fault,

had something to do with the write control settings. The field was written every 500 time steps.

So I got the right values from time step 500 onwards.

It works just as Tom stated. Problem solved!