Hello, for the calculation
 

Hello,

for the calculation of the movement of some boundary points I am doing some calulations on a polyPatch, and I would like to store that data(scalar) somewhere.
I guess, a "surfaceScalarField" would be appropriate, although I only need to store the data for that patch. A "surfaceScalarField" stores the data at the face centres, right?

From there I'd like to interplate those values to the points of the boundary and store that data as well. What is the class to use to store data in boundary points? And how do I do the interpolation, if it's already implemented?

Thank you
markus

If you are storing data for a
 

If you are storing data for a single patch and are not concerned about the patch field type fvPatchField should be used for face-centre data and pointPatchField for vertex data. Both are templated on the type but there are also convenient typedefs for the common types e.g. fvPatchScalarField and pointPatchScalarField.

If I am using a fvPatchScalarF
 

If I am using a fvPatchScalarField it would be constructed with a fvPatch and an internal Field. Where do I get the internal Field from and why does it need one anyways?
thanks
markus

A patch field needs an interna
 

A patch field needs an internal field from which to evaluate the boundary condition. If you do not have a corresponding internal field then you probably should be using scalarField rather than fvPatchScalarField to store your patch data.

Ah, I don't have an correspond
 

Ah, I don't have an corresponding internal field, then I'll use a scalarField for the face centered values.
I could use another scalarField for the corresponding point values and do the interpolation myself. But I would obviously prefer an existing solution for the interpolation. Is there something?
thanks
markus

All done for you and ready to
 

All done for you and ready to use - isn't FOAM wonderful! :-)

Make an object of type primitivePatchInterpolation (or templated PrimitivePatchInterpolation). The functions are in:

~/OpenFOAM/OpenFOAM-1.1/src/OpenFOAM/lnInclude/PrimitivePatchInterpolation.H

and you've got:

//- Interpolate from faces to points
template<class>
tmp<field<type> > faceToPointInterpolate
(
const Field<type>& ff
) const;


//- Interpolate from points to faces
template<class>
tmp<field<type> > pointToFaceInterpolate
(
const Field<type>& pf
) const;

//- Interpolate from faces to edges
template<class>
tmp<field<type> > faceToEdgeInterpolate
(
const Field<type>& ff
) const;

Enjoy (in enery sense of the word!),

Hrv

I'll try that thank you mark
 

I'll try that
thank you
markus