[rando_foamer]

Hi all,

I am wondering how to go about doing the following, and hope someone can help. I've been trying to find a solution using setFields and funkySetFields, but can't find the right approach.

I want to modify the initial condition of a single cell in my geometry, and I want to select this cell based off its proximity to a provided set of coordinates e.g. (x=0.5,y=1.0,z=0.5). This set of coordinates will be close to, but not necessarily directly on, a patch face. For example, given the following simple box as described by this blockMeshDict:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  5                                     |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;

vertices
(   
    (0 0 0)
    (1 0 0) 
    (1 1 0) 
    (0 1 0)
    (0 0 1)
    (1 0 1) 
    (1 1 1) 
    (0 1 1)
);

blocks
(
    hex (0 1 2 3 4 5 6 7) (3 6 100) simpleGrading (1 1 1)
    
);

edges
(
    
);

boundary
(
    inlet
    {
        type patch;
        faces
        (
          (0 1 2 3)
        );
    }
    
    outlet
    {
        type wall;
        faces
        (
          (7 6 5 4)
        );
    }
    
    defaultFaces
    {
        type empty;
        faces ();
    }
    
);

mergePatchPairs
(
);

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

This is obviously a box of dimensions (1 1 1) with a single block.

Ideally I would do this completely in setFields, by finding the cell that has its centre closest to the coordinates (0.5 1.0 0.5), then set its value for my volScalarField (e.g. T). I would not necessarily know what the coordinates were prior to runtime (they would be defined by some other code) and so can't manually create a block specifically for the location.

From what I can gather, there is no "coordinatesToCell" function in setFields, i.e. the choices are:

(
boundaryToFace
boxToCell
boxToFace
boxToPoint
cellToCell
cellToFace
cellToPoint
cylinderAnnulusToCell
cylinderToCell
faceToCell
faceToFace
faceToPoint
faceZoneToCell
faceZoneToFaceZone
fieldToCell
labelToCell
labelToFace
labelToPoint
nbrToCell
nearestToCell
nearestToPoint
normalToFace
patchToFace
pointToCell
pointToFace
pointToPoint
regionToCell
rotatedBoxToCell
setToCellZone
setToFaceZone
setToPointZone
setsToFaceZone
shapeToCell
sphereToCell
surfaceToCell
surfaceToPoint
zoneToCell
zoneToFace
zoneToPoint
)

The closest I can find is the "pointTo*" and "nearestToCell" functions. But from what I understand, I would need to provide a point reference, not coordinates. I don't think I can use "boxToCell" without knowing beforehand what the cell size was, so I didn't accidentally select more than one cell (or zero cells). I'm also not sure what many of the above options actually do (descriptions are very vague in places).

At the moment I am contemplating creating a Python script that finds the face that is nearest to the given coordinates (calculating the average of face points from the polyMesh folder), then using the "faceToCell" function in setFields.

Hopefully there's a better way!

Thanks all for your help.

[Antimony]

Hi,

Doesn't nearestToCell do exactly what you want it to do? From https://github.com/OpenFOAM/OpenFOAM...et/topoSetDict, what it says is this:

// // Cells with cellCentre nearest to coordinates
// source nearestToCell;
// sourceInfo
// {
// points ((0 0 0) (1 1 1)(2 2 2));
// }

So, if you replace the points in the example with your own, should work I think. No?

Cheers,
Antimony

[rando_foamer]

Aha, you are right, of course. I had the syntax wrong, and I misunderstood the error message.

For those interested, the correct syntax to use for the setFieldsDict (rather than topoSetDict) is as follows:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v1812                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      setFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

defaultFieldValues
(
  volScalarFieldValue T 0
);

regions
(
nearestToCell
{
  points ( (0.5 1.0 0.5) );
  fieldValues
    (
      volScalarFieldValue T 1.0
    );
}
);

Thanks Antimony, much appreciated.