[hbulus]

Hello foamers,

I am trying to implement reconCentral scheme from Fe4.0 to OF1812. However i got the compiling error as 'does not match any in class':

wmake libso (reconCentral)
wmakeLnInclude: linking include files to ./lnInclude
Making dependency list for source file reconCentral.C
g++ -std=c++11 -m64 -DOPENFOAM=1812 -Dlinux64 -DWM_ARCH_OPTION=64 -DWM_DP -DWM_LABEL_SIZE=32 -Wall -Wextra -Wold-style-cast -Wnon-virtual-dtor -Wno-unused-parameter -Wno-invalid-offsetof -Wno-attributes -Wno-unknown-pragmas -O3 -DNoRepository -ftemplate-depth-100 -I/opt/apps/OpenFOAM/OpenFOAM-v1812/src/finiteVolume/lnInclude -I/opt/apps/OpenFOAM/OpenFOAM-v1812/src/meshTools/lnInclude -IlnInclude -I. -I/opt/apps/OpenFOAM/OpenFOAM-v1812/src/OpenFOAM/lnInclude -I/opt/apps/OpenFOAM/OpenFOAM-v1812/src/OSspecific/POSIX/lnInclude -fPIC -c reconCentral.C -o Make/linux64GccDPInt32Opt/reconCentral.o
reconCentral.C:37:1: error: prototype for âFoam::tmp<Foam::GeometricField<Type, Foam::fvsPatchField, Foam::surfaceMesh> > Foam::reconCentral<Type>::interpolate(const Foam::GeometricField<Type, Foam::fvPatchField, Foam::volMesh>&, const SFType&) constâ does not match any in class âFoam::reconCentral<Type>â
Foam::reconCentral<Type>::interpolate
^
In file included from reconCentral.C:25:0:
reconCentral.H:142:2: error: candidate is: virtual Foam::tmp<Foam::GeometricField<Type, Foam::fvsPatchField, Foam::surfaceMesh> > Foam::reconCentral<Type>::interpolate(const Foam::GeometricField<Type, Foam::fvPatchField, Foam::volMesh>&) const
interpolate(const GeometricField<Type, fvPatchField, volMesh>&) const;
^
make: *** [Make/linux64GccDPInt32Opt/reconCentral.o] Error 1

I made some obvious modificiations. I share the last version of reconCentral file as attached.

Thanks for every answers.

[cdegroot]

The function signatures in your .H and .C files do not match.

In reconCentral.H:

virtual tmp<GeometricField<Type, fvsPatchField, surfaceMesh> >
	interpolate(const GeometricField<Type, fvPatchField, volMesh>&) const;

In reconCentral.C (neglecting template declarations):

Foam::reconCentral<Type>::interpolate
(
    const GeometricField<Type, fvPatchField, volMesh>& vf,
    //const GeometricField<Type, fvPatchField, volMesh>& sf
    const SFType& sf
) const

In the .H file you have one parameter (the GeometricField object) while in the .C file you have two (the GeometricField object as well as the SFType object). The error is telling you that it can't find a matching class and suggesting the one above in the .H file as a candidate. Not sure exactly what the details of the code are, so I can't suggest which signature is correct, but these will have to be reconciled for the code to compile.

[hbulus]

Originally Posted by cdegroot

The function signatures in your .H and .C files do not match.

In reconCentral.H:

virtual tmp<GeometricField<Type, fvsPatchField, surfaceMesh> >
	interpolate(const GeometricField<Type, fvPatchField, volMesh>&) const;

In reconCentral.C (neglecting template declarations):

Foam::reconCentral<Type>::interpolate
(
    const GeometricField<Type, fvPatchField, volMesh>& vf,
    //const GeometricField<Type, fvPatchField, volMesh>& sf
    const SFType& sf
) const

In the .H file you have one parameter (the GeometricField object) while in the .C file you have two (the GeometricField object as well as the SFType object). The error is telling you that it can't find a matching class and suggesting the one above in the .H file as a candidate. Not sure exactly what the details of the code are, so I can't suggest which signature is correct, but these will have to be reconciled for the code to compile.

When i cancelled the SFType object, nothing has changed. It still gives same error.

[hbulus]

EDIT = Thanks to the friends in this forum, i could modify the reconCentral scheme for OF1812 by their helps. I am sharing the final form of the codes.
This scheme should be used for unstructured meshes with high skewness, especially for tetrahedral cells

reconCentral.C

/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | foam-extend: Open Source CFD
\\ / O peration | Version: 4.0
\\ / A nd | Web: http://www.foam-extend.org
\\/ M anipulation | For copyright notice see file Copyright
-------------------------------------------------------------------------------
License
This file is part of foam-extend.
foam-extend is free software: you can redistribute it and/or modify it
under the terms of the GNU General Public License as published by the
Free Software Foundation, either version 3 of the License, or (at your
option) any later version.
foam-extend is distributed in the hope that it will be useful, but
WITHOUT ANY WARRANTY; without even the implied warranty of
MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE. See the GNU
General Public License for more details.
You should have received a copy of the GNU General Public License
along with foam-extend. If not, see <http://www.gnu.org/licenses/>.
\*---------------------------------------------------------------------------*/

#include "reconCentral.H"
#include "fvMesh.H"

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

template<class Type>
Foam::tmp<Foam::GeometricField<Type, Foam::fvsPatchField, Foam::surfaceMesh> >
Foam::reconCentral<Type>::interpolate
(
const GeometricField<Type, fvPatchField, volMesh>& vf
) const
{
const fvMesh& mesh = this->mesh();

tmp<GeometricField<Type, fvsPatchField, surfaceMesh> > tsf
(
new GeometricField<Type, fvsPatchField, surfaceMesh>
(
IOobject
(
"interpolate("+vf.name()+')',
vf.instance(),
vf.db()
),
mesh,
dimensioned<Type>(vf.name(), vf.dimensions(), pTraits<Type>::zero)
)
);

GeometricField<Type, fvsPatchField, surfaceMesh>& sf = tsf.ref();

const labelList& owner = mesh.owner();
const labelList& neighbour = mesh.neighbour();

const volVectorField& C = mesh.C();
const surfaceVectorField& Cf = mesh.Cf();

tmp
<
GeometricField
<
typename outerProduct<vector, Type>::type,
fvPatchField,
volMesh
>
> tgradVf = gradScheme_().grad(vf);

const GeometricField
<
typename outerProduct<vector, Type>::type,
fvPatchField,
volMesh
>& gradVf = tgradVf();

// Since grad is used on coupled boundaries, correctBoundaryConditions
// needs to be called. HJ, 1/Nov/2012
//gradVf.correctBoundaryConditions();

forAll(sf.internalField(), facei)
{
// Owner contribution
label own = owner[facei];
sf[facei] += 0.5*(vf[own] + ((Cf[facei] - C[own]) & gradVf[own]));

// Neighbour contribution
label nei = neighbour[facei];
sf[facei] += 0.5*(vf[nei] + ((Cf[facei] - C[nei]) & gradVf[nei]));
}


typename GeometricField<Type, fvsPatchField, surfaceMesh>::
Boundary& bSf = sf.boundaryFieldRef();

forAll(bSf, patchi)
{
const fvPatch& p = mesh.boundary()[patchi];

fvsPatchField<Type>& pSf = bSf[patchi];

const labelUList& pOwner = p.faceCells();

const vectorField& pCf = Cf.boundaryField()[patchi];

if (pSf.coupled())
{
Field<Type> vfNei =
vf.boundaryField()[patchi].patchNeighbourField();

Field<typename outerProduct<vector, Type>::type> pGradVfNei =
gradVf.boundaryField()[patchi].patchNeighbourField();

// Build the d-vectors. Used to calculate neighbour face centre
// HJ, 19/Apr/2010
// Better version of d-vectors: Zeljko Tukovic, 25/Apr/2010
vectorField pd = p.delta();

forAll(pOwner, facei)
{

label own = pOwner[facei];

// Owner contribution
pSf[facei] +=
0.5*(vf[own] + ((pCf[facei] - C[own]) & gradVf[own]));

// Neighbour contribution
pSf[facei] +=
0.5*
(
vfNei[facei]
+ (
(pCf[facei] - pd[facei] - C[own])
& pGradVfNei[facei]
)
);
}
}
else if (vf.boundaryField()[patchi].fixesValue())
{
// For fixed boundary patches copy the value
pSf = vf.boundaryField()[patchi];
}
else
{
// For patches that do not fix the value, calculate
// extrapolated field
forAll(pOwner, facei)
{
label own = pOwner[facei];

pSf[facei] =
(vf[own] + ((pCf[facei] - C[own]) & gradVf[own]));
}
}
}

return tsf;
}


template<class Type>
Foam::tmp<Foam::GeometricField<Type, Foam::fvsPatchField, Foam::surfaceMesh> >
Foam::reconCentral<Type>::correction
(
const GeometricField<Type, fvPatchField, volMesh>& vf
) const
{
// Note: Correction is calculated by assembling the complete interpolation
// including extrapolated gradient contribution and subtracting the
// implicit contribution. HJ, 27/Mar/2010
const fvMesh& mesh = this->mesh();

tmp<GeometricField<Type, fvsPatchField, surfaceMesh> > tsfCorr
(
new GeometricField<Type, fvsPatchField, surfaceMesh>
(
IOobject
(
"reconCentralCorrection(" + vf.name() + ')',
mesh.time().timeName(),
mesh,
IOobject::NO_READ,
IOobject::NO_WRITE,
false
),
reconCentral<Type>::interpolate(vf)
- surfaceInterpolationScheme<Type>::interpolate
(
vf,
this->weights()
)
)
);

return tsfCorr;
}


namespace Foam
{
//makelimitedSurfaceInterpolationScheme(reconCentral )
makelimitedSurfaceInterpolationTypeScheme(reconCen tral, scalar)
makelimitedSurfaceInterpolationTypeScheme(reconCen tral, vector)
}

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

[geth03]

@hbulus
i am glad you finally solved your problem
and thanks for sharing your adjustments to the code.