[b.simpson]

Hi,

I am modelling a simple naturally ventilated building where I need to calculate the total CO2 leaving and entering the building through the windows.

I am trying to achieve this by using the surfaceFieldValue function object but I am struggling to get it to select/sample the correct cells. Currently I am using the code below in my controlDict. Does anyone know if you can use the plan type in the sampleSurfaceDict in a way that it doesn't span across the entire model? As I have areas outside of the building which I do not want to include in this.

westValuesSum
    {
        type            surfaceFieldValue;
        libs            ("libfieldFunctionObjects.so");
        log				true;
        writeControl    writeTime;
        writeFields		true;
			
        surfaceFormat   none;
        regionType		sampledSurface;
        name			sum;
        sampledSurfaceDict
        {
            type	plane;
            planeType	pointAndNormal;
            basePoint	(0.05 0 0);
            normalVector	(1 0 0);
        }
			
        operation		sum;

        fields
        (
            CO2
        );
    }

I am using openFOAM v8 with the buoyantSimpleFoam and Spalart-Allmaras turbulence model.

I have also tried using the other two methods (faceSet and patch) for selecting the cells but have been unable to get these to work to a satisfactory level.

Thanks in advance for any help on this issue.

Regards,
Ben

[Swirl]

Hi Ben,

in case your problem still exists, I think you could go a different route than using sampledSurface. Instead, you could define facezones for each window. To do that, you first create a faceSet for the windows with the topoSet command. In the topoSetDict you can specify boxes to define the desired area. In your case, those boxes should probably be very thin in the direction going inside/outside the building.

The topoSetDict options to do thisare explained further here:
https://www.openfoam.com/documentati...boxToFace.html

In the second step you have to covert the faceSet to a faceZone, also using the topoSetDict as described here:
https://www.openfoam.com/documentati...oFaceZone.html

This should create a usable source for your surfaceFieldValue utility.

Hope this helps a little.

[b.simpson]

Thank you for your reply.

I agree that the faceSet/faceZone is the way to go for what I am trying to achieve.

In case anyone is interested I got it to work on my model by creating a cellSet from an stl file that I generated in blender. I then created a faceSet and faceZone from this. I was then able to use the faceZone for the surfaceFieldValue.

Below is the setup I used.

topoSetDict:

{
        name    southCell;
        type    cellSet;
        action  new;
		source surfaceToCell;
		sourceInfo
		{
			file            "$FOAM_CASE/constant/triSurface/sWin.stl";
			useSurfaceOrientation false;  
			outsidePoints   ((1 1 1));    // definition of outside
			includeCut      true;              // cells cut by surface
			includeInside   false;              // cells not on outside of surf
			includeOutside  false;              // cells on outside of surf
			nearDistance    -1;                 // cells with centre near surf
												// (set to -1 if not used)
			curvature       -100;                // cells within nearDistance
												// and near surf curvature
												// (set to -100 if not used)
		}
}
{
        name    southFace;
        type    faceSet;
        action  new;
        source  cellToFace;
		sourceInfo
		{
			set     southCell;
			option	all;
		}
}
{
        name    southZone;
        type    faceZoneSet;
        action  new;
        source  setToFaceZone;
		sourceInfo
		{
			faceSet	southFace;
		}
}

controlDict:

surfaceInterpolate_CO2
		{
			 type        surfaceInterpolate;
			 libs        ("libfieldFunctionObjects.so");
			 fields      
			 (
				 (CO2 CO2Interp)
			 ); 
			 executeControl  writeTime;
			 writeControl    writeTime;   
		}

southSumPos
		{
			type            surfaceFieldValue;
			libs            ("libfieldFunctionObjects.so");
			log				true;
			executeControl  writeTime;
			writeControl    writeTime;
			writeFields		true;
			
			surfaceFormat   none;
			regionType		faceZone;
			name			southZone;
			
			operation		sumDirection;
			direction		(0 1 0);

			fields
			(
				CO2Interp
			);
		}

Hope this is helpful for anyone using the surfaceFieldValue function objects.

Regards,
Ben