[praveensrikanth91]

Hello Forum users,

I am working with the conjugate heat transfer solver where I am trying to find the temperature at a liquid vapor interface by interpolating the temperatures from the liquid and the gas regions and taking an average. I interpolate the temperatures with

surfaceScalarField TI_liquid = fvc::interpolate(liquidT); 
surfaceScalarField TI_gas = fvc::interpolate(gasT);

but this does it for the entire region. I also know the cells next to the boundary which I get using the respective patchIDs

const labelList& gasPFaceCells = gasMesh_.boundary()[gasPatchID_].faceCells();

But I am not sure how to find the face IDs for the boundary faces for these cells which I can then use to get the interpolated temperature at the boundary. I have been going through this forum without much luck so any help is most appreciated

[vigneshTG]

Hi,
If you have not figured it out,

//To access the mesh information for the boundary
const polyPatch& cPatch = mesh.boundaryMesh()[patchI];

//Starting index of the face in a patch
label faceId_start = cPatch.start() ;

List of cells close to a boundary
const labelUList& faceCells = cPatch.faceCells();

forAll(cPatch, faceI) 
{ 
  
// index of each face
label faceID = faceId_start +faceI;

//id of the owner cell having the face
label faceOwner = faceCells[faceI] ;

....

 }

If there is a better way, do let me know !!

[praveensrikanth91]

Hey Vignesh,

Thank you so much for that. I did not realise that the face numbers on the patch were going to be continuous.

	const cell& gasFaces = gasMesh_.cells()[gasPfCellI];
	label gasfaceI = 0;

	forAll(gasFaces, i)
	{
		label gasPatchI = gasMesh_.boundaryMesh().whichPatch(gasFaces[i]);
		if(gasPatchI == gasPatchID_)
		{
			gasfaceI = gasFaces[i];
			Info<<"gasFaceI = "<< gasfaceI<<endl;
		}
	}

I used boundary().faceCells() on the boundary patches to get the cells on the boundary like you did. It seems to work fine as far as I can see. I will let you know if I find something wrong with it. Thanks again.