[AlmostSurelyRob]

Dear Users and Developers,

it is possible in OpenFOAM to set up a monitoring boundary? I am trying to do some runtime post-processing. I would be satisifed with one of the two solutions

1) Calculate a surface integral on a given set of faces
2) Interpolate field values for a set of faces

According to this link
http://www.openfoam.com/features/run...processing.php
my request would be satisifed by either fieldValue and surfaceInterpolateFields.

Using setSet I have already defined the correct face sets and confirmed their validity with paraview. I am only interested in phase indicator field from a VOF simulation.

First problem: fieldValue doesn't appear to be implemented or registered.

Unknown function type fieldValue

Valid functions are : 

14
(
cellSource
faceSource
fieldAverage
fieldCoordinateSystemTransform
fieldMinMax
nearWallFields
patchProbes
probes
readFields
regionSizeDistribution
sets
streamLine
surfaceInterpolateFields
surfaces
)

Second problem surfaceInterpolate defined in the following way in controlDict

functions
{

  monitoring1
  {
    type            fieldValue;
    functionObjectLibs ( "libfieldFunctionObjects.so" );
    outputControl   timeStep;
    patches monitoringSurface1;
    fields ((alpha1 alpha1Near));
  }
}

produces output that does not match my exectations. What is actually alpha1Near? How do I tell surfacInterpolate that I only want interoplation on a surface given by a faceSet that resides in constant/polyMesh/sets?

Could anyone explain to me what is the correct syntax for defining this function and how could I use it to achieve my goal?

In the worst case I would like to point out that the above website needs updating (fieldValue absent?). Please do let me know if you understand how it is supposed to work.

[AlmostSurelyRob]

I've just discovered that cuttingPlane could do what I want from interpolateSurfaceFields, but alas it crashes with my periodic domain producing no output at all. It's strange because the plane does not pass through a periodic patch.

functions
{

  cuttingPlane
  {
    type            surfaces;
    functionObjectLibs ("libsampling.so");
    outputControl   timeStep;

    surfaceFormat   vtk;
    fields          (alpha1);

    interpolationScheme cellPoint;

    surfaces
      (
       monitoring1
       {
       type            cuttingPlane;
       planeType       pointAndNormal;
       pointAndNormalDict
       {
       basePoint       (0 0 0.6);
       normalVector    (0 0 1);
       }
       interpolate     true;
       }
      );
  }

}

and the error

Unhandled coupledPolyPatch type cyclic

    From function isoSurface::collocatedFaces(const coupledPolyPatch&) const
    in file sampledSurface/isoSurface/isoSurface.C at line 97.

FOAM aborting

is that normal?

Also I don't know if VTK will be any useful. I just want to take a signal out of it which will be the integrated volume fraction. Will I be able to do it efficiently with plenty of VTK files?

[AlmostSurelyRob]

Praise be to swak4Foam developers!

Using this link
http://www.cfd-online.com/Forums/ope...e-average.html
I figured out that this piece of code in my controlDict

libs (
"libOpenFOAM.so"
"libsimpleSwakFunctionObjects.so" 
"libswakFunctionObjects.so"
);

functions
{
  liquidHoldup1
  {
    type            swakExpression;
    valueType       surface;
    surfaceName monitoringBoundary1;
    surface {
            type plane;
            basePoint       (0 0 0.6);
            normalVector    (0 0 1);
            interpolate false;
        }
    functionObjectLibs ("libsampling.so");
    outputControl   timeStep;

    zoneName monitoringZone1;
    accumulations ( min);
    expression "sum((1-alpha1)*area())/sum(area())";
    verbose true;
  }
}

dooes the job for point 1 of my querry. I am still cuious to learn how to do point 2.

[gschaider]

Originally Posted by AlmostSurelyRob

Praise be to swak4Foam developers!

Using this link
http://www.cfd-online.com/Forums/ope...e-average.html
I figured out that this piece of code in my controlDict

<code snipped>

does the job for point 1 of my querry. I am still cuious to learn how to do point 2.

That would be "Interpolate field values for a set of faces"? With "set of faces" you mean a faceSet or a faceZone? As you already bit the bullet and installed swak I can offer you this: swakExpressions that work on faceSets or faceZones have an option "autoInterpolate". If you set the to true and use the name of a field that is defined on the cells in your expression the field is automatically interpolated onto the faces and used for the calculation. Other option would be to use an expressionField-functionObject that generates (for instance) a field pOnFaces from the expression "interpolate(p)" and use that with one of the stock function objects