diff --git a/src/fvOptions/Make/files b/src/fvOptions/Make/files
index 889ddebabb8d09aecf0d3468a589e85f329665e7..9a8376a95cd20672f6f6037df3ced67776fc5cae 100644
--- a/src/fvOptions/Make/files
+++ b/src/fvOptions/Make/files
@@ -22,6 +22,8 @@ $(derivedSources)/directionalPressureGradientExplicitSource/directionalPressureG
$(derivedSources)/directionalPressureGradientExplicitSource/directionalPressureGradientExplicitSourceIO.C
$(derivedSources)/effectivenessHeatExchangerSource/effectivenessHeatExchangerSource.C
$(derivedSources)/explicitPorositySource/explicitPorositySource.C
+$(derivedSources)/jouleHeatingSource/jouleHeatingSource.C
+$(derivedSources)/jouleHeatingSource/jouleHeatingSourceIO.C
$(derivedSources)/meanVelocityForce/meanVelocityForce.C
$(derivedSources)/meanVelocityForce/meanVelocityForceIO.C
$(derivedSources)/meanVelocityForce/patchMeanVelocityForce/patchMeanVelocityForce.C
diff --git a/src/fvOptions/sources/derived/jouleHeatingSource/jouleHeatingSource.C b/src/fvOptions/sources/derived/jouleHeatingSource/jouleHeatingSource.C
new file mode 100644
index 0000000000000000000000000000000000000000..7a7a8ccde7db991d1bea27b65168f93b0cf3db3c
--- /dev/null
+++ b/src/fvOptions/sources/derived/jouleHeatingSource/jouleHeatingSource.C
@@ -0,0 +1,215 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2016-2017 OpenCFD Ltd.
+ \\/ M anipulation |
+-------------------------------------------------------------------------------
+License
+ This file is part of OpenFOAM.
+
+ OpenFOAM 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.
+
+ OpenFOAM 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 OpenFOAM. If not, see <http://www.gnu.org/licenses/>.
+
+\*---------------------------------------------------------------------------*/
+
+#include "jouleHeatingSource.H"
+#include "fvMatrices.H"
+#include "fvmLaplacian.H"
+#include "fvcGrad.H"
+#include "zeroGradientFvPatchField.H"
+#include "basicThermo.H"
+#include "addToRunTimeSelectionTable.H"
+
+// * * * * * * * * * * * * * Static Member Functions * * * * * * * * * * * * //
+
+namespace Foam
+{
+namespace fv
+{
+ defineTypeNameAndDebug(jouleHeatingSource, 0);
+
+ addToRunTimeSelectionTable
+ (
+ option,
+ jouleHeatingSource,
+ dictionary
+ );
+}
+}
+
+
+const Foam::word Foam::fv::jouleHeatingSource::sigmaName(typeName + ":sigma");
+
+
+// * * * * * * * * * * * * * Private Member Functions * * * * * * * * * * * //
+
+const Foam::coordinateSystem& Foam::fv::jouleHeatingSource::coordSys() const
+{
+ if (!coordSysPtr_.valid())
+ {
+ FatalErrorInFunction
+ << "Co-ordinate system invalid"
+ << abort(FatalError);
+ }
+
+ return coordSysPtr_();
+}
+
+
+Foam::tmp<Foam::volSymmTensorField>
+Foam::fv::jouleHeatingSource::transformSigma
+(
+ const volVectorField& sigmaLocal
+) const
+{
+ tmp<volSymmTensorField> tsigma
+ (
+ new volSymmTensorField
+ (
+ IOobject
+ (
+ sigmaName,
+ mesh_.time().timeName(),
+ mesh_,
+ IOobject::NO_READ,
+ IOobject::NO_WRITE,
+ false
+ ),
+ mesh_,
+ dimensionedSymmTensor("0", sigmaLocal.dimensions(), Zero),
+ zeroGradientFvPatchField<symmTensor>::typeName
+ )
+ );
+
+ volSymmTensorField& sigma = tsigma.ref();
+ sigma.primitiveFieldRef() = coordSys().R().transformVector(sigmaLocal);
+
+ sigma.correctBoundaryConditions();
+
+ return tsigma;
+}
+
+
+// * * * * * * * * * * * * * * * * Constructors * * * * * * * * * * * * * * //
+
+Foam::fv::jouleHeatingSource::jouleHeatingSource
+(
+ const word& sourceName,
+ const word& modelType,
+ const dictionary& dict,
+ const fvMesh& mesh
+)
+:
+ option(sourceName, modelType, dict, mesh),
+ TName_("T"),
+ V_
+ (
+ IOobject
+ (
+ typeName + ":V",
+ mesh.time().timeName(),
+ mesh,
+ IOobject::MUST_READ,
+ IOobject::AUTO_WRITE
+ ),
+ mesh
+ ),
+ anisotropicElectricalConductivity_(false),
+ scalarSigmaVsTPtr_(nullptr),
+ vectorSigmaVsTPtr_(nullptr),
+ coordSysPtr_(nullptr),
+ curTimeIndex_(-1)
+{
+ // Set the field name to that of the energy field from which the temperature
+ // is obtained
+
+ const basicThermo& thermo =
+ mesh_.lookupObject<basicThermo>(basicThermo::dictName);
+
+ fieldNames_.setSize(1, thermo.he().name());
+
+ applied_.setSize(fieldNames_.size(), false);
+
+ read(dict);
+}
+
+
+// * * * * * * * * * * * * * * * * Destructor * * * * * * * * * * * * * * * //
+
+Foam::fv::jouleHeatingSource::~jouleHeatingSource()
+{}
+
+
+// * * * * * * * * * * * * * * * * Destructor * * * * * * * * * * * * * * * //
+
+void Foam::fv::jouleHeatingSource::addSup
+(
+ const volScalarField& rho,
+ fvMatrix<scalar>& eqn,
+ const label fieldi
+)
+{
+ DebugInfo<< name() << ": applying source to " << eqn.psi().name() << endl;
+
+ if (curTimeIndex_ != mesh_.time().timeIndex())
+ {
+ if (anisotropicElectricalConductivity_)
+ {
+ // Update sigma as a function of T if required
+ const volVectorField& sigmaLocal = updateSigma(vectorSigmaVsTPtr_);
+
+ tmp<volSymmTensorField> sigma = transformSigma(sigmaLocal);
+
+ // Solve the electrical potential equation
+ fvScalarMatrix VEqn(fvm::laplacian(sigma, V_));
+ VEqn.relax();
+ VEqn.solve();
+ }
+ else
+ {
+ // Update sigma as a function of T if required
+ const volScalarField& sigma = updateSigma(scalarSigmaVsTPtr_);
+
+ // Solve the electrical potential equation
+ fvScalarMatrix VEqn(fvm::laplacian(sigma, V_));
+ VEqn.relax();
+ VEqn.solve();
+ }
+
+ curTimeIndex_ = mesh_.time().timeIndex();
+ }
+
+ // Add the Joule heating contribution
+
+ const volVectorField gradV(fvc::grad(V_));
+ if (anisotropicElectricalConductivity_)
+ {
+ const volVectorField& sigmaLocal =
+ mesh_.lookupObject<volVectorField>(sigmaName);
+
+ tmp<volSymmTensorField> sigma = transformSigma(sigmaLocal);
+
+ eqn += (sigma & gradV) & gradV;
+ }
+ else
+ {
+ const volScalarField& sigma =
+ mesh_.lookupObject<volScalarField>(sigmaName);
+
+ eqn += (sigma*gradV) & gradV;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/src/fvOptions/sources/derived/jouleHeatingSource/jouleHeatingSource.H b/src/fvOptions/sources/derived/jouleHeatingSource/jouleHeatingSource.H
new file mode 100644
index 0000000000000000000000000000000000000000..58565647393f01904d4fc9e8e25be88cc09b99ce
--- /dev/null
+++ b/src/fvOptions/sources/derived/jouleHeatingSource/jouleHeatingSource.H
@@ -0,0 +1,278 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2016-2017 OpenCFD Ltd.
+ \\/ M anipulation |
+-------------------------------------------------------------------------------
+License
+ This file is part of OpenFOAM.
+
+ OpenFOAM 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.
+
+ OpenFOAM 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 OpenFOAM. If not, see <http://www.gnu.org/licenses/>.
+
+Class
+ Foam::fv::jouleHeatingSource
+
+Group
+ grpFvOptionsSources
+
+Description
+ Evolves an electrical potential equation
+
+ \f[
+ \grad \left( \sigma \grad V \right)
+ \f]
+
+ where \f$ V \f$ is electrical potential and \f$\sigma\f$ is the
+ electrical current
+
+ To provide a Joule heating contribution according to:
+
+ Differential form of Joule heating - power per unit volume:
+
+ \f[
+ \frac{d(P)}{d(V)} = J \cdot E
+ \f]
+
+ where \f$ J \f$ is the current density and \f$ E \f$ the electric field.
+ If no magnetic field is present:
+
+ \f[
+ J = \sigma E
+ \f]
+
+ The electric field given by
+
+ \f[
+ E = \grad V
+ \f]
+
+ Therefore:
+
+ \f[
+ \frac{d(P)}{d(V)} = J \cdot E
+ = (sigma E) \cdot E
+ = (sigma \grad V) \cdot \grad V
+ \f]
+
+
+Usage
+ Isotropic (scalar) electrical conductivity
+ \verbatim
+ jouleHeatingSourceCoeffs
+ {
+ anisotropicElectricalConductivity no;
+
+ // Optionally specify the conductivity as a function of temperature
+ // Note: if not supplied, this will be read from the time directory
+ sigma table
+ (
+ (273 1e5)
+ (1000 1e5)
+ );
+ }
+ \endverbatim
+
+ Anisotropic (vectorial) electrical conductivity
+ jouleHeatingSourceCoeffs
+ {
+ anisotropicElectricalConductivity yes;
+
+ coordinateSystem
+ {
+ type cartesian;
+ origin (0 0 0);
+
+ coordinateRotation
+ {
+ type axesRotation;
+ e1 (1 0 0);
+ e3 (0 0 1);
+ }
+ }
+
+ // Optionally specify sigma as a function of temperature
+ //sigma (31900 63800 127600);
+ //
+ //sigma table
+ //(
+ // (0 (0 0 0))
+ // (1000 (127600 127600 127600))
+ //);
+ }
+
+
+ Where:
+ \table
+ Property | Description | Required | Default value
+ T | Name of temperature field | no | T
+ sigma | Electrical conductivity as a function of temperature |no|
+ anisotropicElectricalConductivity | Anisotropic flag | yes |
+ \endtable
+
+ The electrical conductivity can be specified using either:
+ - If the \c sigma entry is present the electrical conductivity is specified
+ as a function of temperature using a Function1 type
+ - If not present the sigma field will be read from file
+ - If the anisotropicElectricalConductivity flag is set to 'true', sigma
+ should be specified as a vector quantity
+
+SourceFiles
+ jouleHeatingSource.C
+
+SeeAlso
+ Foam::Function1
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef fv_jouleHeatingSource_H
+#define fv_jouleHeatingSource_H
+
+#include "fvOption.H"
+#include "Function1.H"
+#include "coordinateSystem.H"
+#include "volFields.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+namespace fv
+{
+
+/*---------------------------------------------------------------------------*\
+ Class jouleHeatingSource Declaration
+\*---------------------------------------------------------------------------*/
+
+class jouleHeatingSource
+:
+ public option
+{
+ // Private data
+
+ //- Name of electrical conductivity field
+ static const word sigmaName;
+
+ //- Name of temperature field - default = "T" (optional)
+ word TName_;
+
+ //- Electrical potential field / [V]
+ volScalarField V_;
+
+ //- Flag to indicate that the electrical conductivity is anisotropic
+ bool anisotropicElectricalConductivity_;
+
+ //- Electrical conductivity as a scalar function of temperature
+ autoPtr<Function1<scalar>> scalarSigmaVsTPtr_;
+
+ //- Electrical conductivity as a vector function of temperature
+ autoPtr<Function1<vector>> vectorSigmaVsTPtr_;
+
+ //- Co-ordinate system - used for vectorial electrical conductivity
+ autoPtr<coordinateSystem> coordSysPtr_;
+
+ //- Current time index (used for updating)
+ label curTimeIndex_;
+
+
+ // Private Member Functions
+
+ //- Disallow default bitwise copy construct
+ jouleHeatingSource(const jouleHeatingSource&);
+
+ //- Disallow default bitwise assignment
+ void operator=(const jouleHeatingSource&);
+
+ //- Return the co-ordinate system for anisotropic electrical
+ // conductivity
+ const coordinateSystem& coordSys() const;
+
+ //- Transform the anisotropic electrical conductivity into global system
+ tmp<volSymmTensorField> transformSigma
+ (
+ const volVectorField& sigmaLocal
+ ) const;
+
+ //- Initialise the electrical conductivity field
+ template<class Type>
+ void initialiseSigma
+ (
+ const dictionary& dict,
+ autoPtr<Function1<Type>>& sigmaVsTPtr
+ );
+
+ //- Update the electrical conductivity field
+ template<class Type>
+ const GeometricField<Type, fvPatchField, volMesh>&
+ updateSigma(const autoPtr<Function1<Type>>& sigmaVsTPtr) const;
+
+
+public:
+
+ //- Runtime type information
+ TypeName("jouleHeatingSource");
+
+
+ // Constructors
+
+ //- Construct from explicit source name and mesh
+ jouleHeatingSource
+ (
+ const word& sourceName,
+ const word& modelType,
+ const dictionary& dict,
+ const fvMesh& mesh
+ );
+
+
+ //- Destructor
+ virtual ~jouleHeatingSource();
+
+
+ // Member Functions
+
+ // Evaluate
+
+ //- Add explicit contribution to compressible momentum equation
+ virtual void addSup
+ (
+ const volScalarField& rho,
+ fvMatrix<scalar>& eqn,
+ const label fieldi
+ );
+
+
+ // IO
+
+ //- Read source dictionary
+ virtual bool read(const dictionary& dict);
+};
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace fv
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#ifdef NoRepository
+ #include "jouleHeatingSourceTemplates.C"
+#endif
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //
diff --git a/src/fvOptions/sources/derived/jouleHeatingSource/jouleHeatingSourceIO.C b/src/fvOptions/sources/derived/jouleHeatingSource/jouleHeatingSourceIO.C
new file mode 100644
index 0000000000000000000000000000000000000000..ce4dde6f95ee0c2b9fd5cc807e0ce638b5639f38
--- /dev/null
+++ b/src/fvOptions/sources/derived/jouleHeatingSource/jouleHeatingSourceIO.C
@@ -0,0 +1,59 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2016-2017 OpenCFD Ltd.
+ \\/ M anipulation |
+-------------------------------------------------------------------------------
+License
+ This file is part of OpenFOAM.
+
+ OpenFOAM 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.
+
+ OpenFOAM 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 OpenFOAM. If not, see <http://www.gnu.org/licenses/>.
+
+\*---------------------------------------------------------------------------*/
+
+#include "jouleHeatingSource.H"
+
+// * * * * * * * * * * * * * Private Member Functions * * * * * * * * * * * //
+
+bool Foam::fv::jouleHeatingSource::read(const dictionary& dict)
+{
+ if (option::read(dict))
+ {
+ coeffs_.readIfPresent("T", TName_);
+ coeffs_.lookup("anisotropicElectricalConductivity")
+ >> anisotropicElectricalConductivity_;
+
+ if (anisotropicElectricalConductivity_)
+ {
+ Info<< " Using vector electrical conductivity" << endl;
+
+ initialiseSigma(coeffs_, vectorSigmaVsTPtr_);
+ coordSysPtr_ = coordinateSystem::New(mesh_, coeffs_);
+ }
+ else
+ {
+ Info<< " Using scalar electrical conductivity" << endl;
+
+ initialiseSigma(coeffs_, scalarSigmaVsTPtr_);
+ }
+
+ return true;
+ }
+
+ return false;
+}
+
+
+// ************************************************************************* //
diff --git a/src/fvOptions/sources/derived/jouleHeatingSource/jouleHeatingSourceTemplates.C b/src/fvOptions/sources/derived/jouleHeatingSource/jouleHeatingSourceTemplates.C
new file mode 100644
index 0000000000000000000000000000000000000000..11d7eed98c6ef912f4422511220ff3208686ec42
--- /dev/null
+++ b/src/fvOptions/sources/derived/jouleHeatingSource/jouleHeatingSourceTemplates.C
@@ -0,0 +1,147 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2016-2017 OpenCFD Ltd.
+ \\/ M anipulation |
+-------------------------------------------------------------------------------
+License
+ This file is part of OpenFOAM.
+
+ OpenFOAM 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.
+
+ OpenFOAM 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 OpenFOAM. If not, see <http://www.gnu.org/licenses/>.
+
+\*---------------------------------------------------------------------------*/
+
+#include "emptyFvPatchField.H"
+
+template<class Type>
+void Foam::fv::jouleHeatingSource::initialiseSigma
+(
+ const dictionary& dict,
+ autoPtr<Function1<Type>>& sigmaVsTPtr
+)
+{
+ typedef GeometricField<Type, fvPatchField, volMesh> VolFieldType;
+
+ if (dict.found("sigma"))
+ {
+ // Sigma to be defined using a Funcion1 type
+ sigmaVsTPtr = Function1<Type>::New("sigma", dict);
+
+ tmp<VolFieldType> tsigma
+ (
+ new VolFieldType
+ (
+ IOobject
+ (
+ typeName + ":sigma",
+ mesh_.time().timeName(),
+ mesh_,
+ IOobject::NO_READ,
+ IOobject::AUTO_WRITE
+ ),
+ mesh_,
+ dimensioned<Type>
+ (
+ "0",
+ sqr(dimCurrent)/dimPower/dimLength,
+ Zero
+ )
+ )
+ );
+
+ mesh_.objectRegistry::store(tsigma.ptr());
+
+ Info<< " Conductivity 'sigma' read from dictionary as f(T)"
+ << nl << endl;
+ }
+ else
+ {
+ // Sigma to be defined by user input
+ tmp<VolFieldType> tsigma
+ (
+ new VolFieldType
+ (
+ IOobject
+ (
+ typeName + ":sigma",
+ mesh_.time().timeName(),
+ mesh_,
+ IOobject::MUST_READ,
+ IOobject::AUTO_WRITE
+ ),
+ mesh_
+ )
+ );
+
+ mesh_.objectRegistry::store(tsigma.ptr());
+
+ Info<< " Conductivity 'sigma' read from file" << nl << endl;
+ }
+}
+
+
+template<class Type>
+const Foam::GeometricField<Type, Foam::fvPatchField, Foam::volMesh>&
+Foam::fv::jouleHeatingSource::updateSigma
+(
+ const autoPtr<Function1<Type>>& sigmaVsTPtr
+) const
+{
+ typedef GeometricField<Type, fvPatchField, volMesh> VolFieldType;
+
+ VolFieldType& sigma =
+ const_cast<VolFieldType&>
+ (
+ mesh_.lookupObject<VolFieldType>(typeName + ":sigma")
+ );
+
+ if (!sigmaVsTPtr.valid())
+ {
+ // Electrical conductivity field, sigma, was specified by the user
+ return sigma;
+ }
+
+ const volScalarField& T = mesh_.lookupObject<volScalarField>(TName_);
+
+ // Internal field
+ forAll(sigma, i)
+ {
+ sigma[i] = sigmaVsTPtr->value(T[i]);
+ }
+
+
+ // Boundary field
+ typename VolFieldType::Boundary& bf = sigma.boundaryFieldRef();
+ forAll(bf, patchi)
+ {
+ fvPatchField<Type>& pf = bf[patchi];
+ if (!isA<emptyFvPatchField<Type>>(pf))
+ {
+ const scalarField& Tbf = T.boundaryField()[patchi];
+ forAll(pf, facei)
+ {
+ pf[facei] = sigmaVsTPtr->value(Tbf[facei]);
+ }
+ }
+ }
+
+ // Update processor patches
+ sigma.correctBoundaryConditions();
+
+ return sigma;
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/0.orig/solid/T b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/0.orig/solid/T
new file mode 100644
index 0000000000000000000000000000000000000000..302392cd2cb9d078fd840f16e39aba279492d901
--- /dev/null
+++ b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/0.orig/solid/T
@@ -0,0 +1,49 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1612+ |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0/solid";
+ object T;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [ 0 0 0 1 0 0 0 ];
+
+internalField uniform 500;
+
+boundaryField
+{
+ left
+ {
+ type fixedValue;
+ value uniform 500;
+ }
+ right
+ {
+ type fixedValue;
+ value uniform 500;
+ }
+ top
+ {
+ type zeroGradient;
+ }
+ bottom
+ {
+ type zeroGradient;
+ }
+ frontAndBack
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/0.orig/solid/jouleHeatingSource:V b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/0.orig/solid/jouleHeatingSource:V
new file mode 100644
index 0000000000000000000000000000000000000000..407005dbd410f993be2fa147e144f63d8e00281b
--- /dev/null
+++ b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/0.orig/solid/jouleHeatingSource:V
@@ -0,0 +1,49 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1612+ |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0/heater";
+ object jouleHeatingSource:V;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [ 1 2 -3 0 0 -1 0 ];
+
+internalField uniform 0;
+
+boundaryField
+{
+ left
+ {
+ type fixedValue;
+ value uniform 1.5;
+ }
+ right
+ {
+ type fixedValue;
+ value uniform 0;
+ }
+ top
+ {
+ type zeroGradient;
+ }
+ bottom
+ {
+ type zeroGradient;
+ }
+ frontAndBack
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/0.orig/solid/jouleHeatingSource:sigma b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/0.orig/solid/jouleHeatingSource:sigma
new file mode 100644
index 0000000000000000000000000000000000000000..b3acde6b3665c798eb5bd0aabecb0df601553d39
--- /dev/null
+++ b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/0.orig/solid/jouleHeatingSource:sigma
@@ -0,0 +1,47 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1612+ |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0/heater";
+ object jouleHeatingSource:sigma;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [ -1 -3 3 0 0 2 0 ];
+
+internalField uniform 127599.8469;
+
+boundaryField
+{
+ left
+ {
+ type zeroGradient;
+ }
+ right
+ {
+ type zeroGradient;
+ }
+ top
+ {
+ type zeroGradient;
+ }
+ bottom
+ {
+ type zeroGradient;
+ }
+ frontAndBack
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/0.orig/solid/p b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/0.orig/solid/p
new file mode 100644
index 0000000000000000000000000000000000000000..d0b8fa4f65eaa44367c142cbf6c7894c0090a632
--- /dev/null
+++ b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/0.orig/solid/p
@@ -0,0 +1,36 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1612+ |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0/solid";
+ object p;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [1 -1 -2 0 0 0 0];
+
+internalField uniform 100000;
+
+boundaryField
+{
+ ".*"
+ {
+ type calculated;
+ value uniform 100000;
+ }
+ frontAndBack
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/Allclean b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/Allclean
new file mode 100755
index 0000000000000000000000000000000000000000..31c0b764b5a135ceb1891ba7d5dda8123cb51ded
--- /dev/null
+++ b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/Allclean
@@ -0,0 +1,14 @@
+#!/bin/sh
+cd ${0%/*} || exit 1 # Run from this directory
+
+# Source tutorial clean functions
+. $WM_PROJECT_DIR/bin/tools/CleanFunctions
+
+cleanCase
+rm -rf 0
+
+foamCleanPolyMesh -region solid
+
+rm -f *.OpenFOAM OF_vs_ANALYTICAL.eps
+
+#------------------------------------------------------------------------------
diff --git a/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/Allrun b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/Allrun
new file mode 100755
index 0000000000000000000000000000000000000000..98857416a91cbba898dc7c53731e2306b08af098
--- /dev/null
+++ b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/Allrun
@@ -0,0 +1,13 @@
+#!/bin/sh
+cd ${0%/*} || exit 1 # Run from this directory
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+
+./Allrun.pre
+
+runApplication $(getApplication)
+
+./createGraphs
+
+# -----------------------------------------------------------------------------
diff --git a/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/Allrun-parallel b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/Allrun-parallel
new file mode 100755
index 0000000000000000000000000000000000000000..b48e4c119d991666fbaa5898f239939af8a88f90
--- /dev/null
+++ b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/Allrun-parallel
@@ -0,0 +1,17 @@
+#!/bin/sh
+cd ${0%/*} || exit 1 # Run from this directory
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+
+./Allrun.pre
+
+runApplication -s solid decomposePar -region solid
+
+runParallel $(getApplication)
+
+runApplication -s solid reconstructPar -latestTime -region solid
+
+./createGraphs
+
+# -----------------------------------------------------------------------------
diff --git a/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/Allrun.pre b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/Allrun.pre
new file mode 100755
index 0000000000000000000000000000000000000000..c8198f9848a5385a6251bd757cbee53fa0ed6398
--- /dev/null
+++ b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/Allrun.pre
@@ -0,0 +1,15 @@
+#!/bin/sh
+cd ${0%/*} || exit 1 # Run from this directory
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+
+# Create meshe
+runApplication -s solid blockMesh -region solid
+
+# create dummy files for post-processing
+paraFoam -touch -region solid
+
+restore0Dir
+
+# -----------------------------------------------------------------------------
diff --git a/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/constant/regionProperties b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/constant/regionProperties
new file mode 100644
index 0000000000000000000000000000000000000000..4b0d4cf1d548510b21558fdebebb15562da22a53
--- /dev/null
+++ b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/constant/regionProperties
@@ -0,0 +1,24 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: plus |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "constant";
+ object regionProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+regions
+(
+ fluid ()
+ solid (solid)
+);
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/constant/solid/thermophysicalProperties b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/constant/solid/thermophysicalProperties
new file mode 100644
index 0000000000000000000000000000000000000000..a24fa3e3ab72e2e13fccba9fb102b26c43802341
--- /dev/null
+++ b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/constant/solid/thermophysicalProperties
@@ -0,0 +1,54 @@
+/*--------------------------------*- C++ -*----------------------------------* \
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: plus |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object thermophysicalProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+thermoType
+{
+ type heSolidThermo;
+ mixture pureMixture;
+ transport constIso;
+ thermo hConst;
+ equationOfState rhoConst;
+ specie specie;
+ energy sensibleEnthalpy;
+}
+
+mixture
+{
+ specie
+ {
+ nMoles 1;
+ molWeight 12;
+ }
+
+ transport
+ {
+ kappa 200;
+ }
+
+ thermodynamics
+ {
+ Hf 0;
+ Cp 700;
+ }
+
+ equationOfState
+ {
+ rho 8000;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/createGraphs b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/createGraphs
new file mode 100755
index 0000000000000000000000000000000000000000..04bbc57ea0a4109b12822ba42e3cac767d0ef9ea
--- /dev/null
+++ b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/createGraphs
@@ -0,0 +1,87 @@
+#!/bin/sh
+#------------------------------------------------------------------------------
+# ========= |
+# \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+# \\ / O peration |
+# \\ / A nd | Copyright (C) 2017 OpenCFD Ltd.
+# \\/ M anipulation |
+#-------------------------------------------------------------------------------
+# License
+# This file is part of OpenFOAM.
+#
+# OpenFOAM 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.
+#
+# OpenFOAM 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 OpenFOAM. If not, see <http://www.gnu.org/licenses/>.
+#
+# Script
+# createGraphs
+#
+# Description
+# Creates .eps graph of OpenFOAM results vs analytical solution for the
+# Joule heating case
+#
+#------------------------------------------------------------------------------
+
+cd ${0%/*} || exit 1 # Run from this directory
+
+# Stop on first error
+set -e
+
+# test if gnuplot exists on the system
+if ! which gnuplot > /dev/null 2>&1
+then
+ echo "FOAM FATAL ERROR: gnuplot not found - skipping graph creation" >&2
+ exit 1
+fi
+
+
+echo "Creating graph"
+OFDATA='postProcessing/sample1/solid/20000/centreLine_T_jouleHeatingSource:V_jouleHeatingSource:sigma.xy'
+
+if [ ! -f "$OFDATA" ]
+then
+ echo "FOAM FATAL ERROR: OpenFOAM results not available in $OFDATA" >&2
+ exit 1
+fi
+
+gnuplot<<EOF
+set terminal postscript eps color enhanced
+set output "OF_vs_ANALYTICAL.eps"
+set xlabel "Length, x / [m]"
+set ylabel "Temperature / [K]"
+set grid
+set key left top
+rho = 7.837e-6
+sigma = 1/rho
+kappa = 200
+L = 2.5
+D = 0.1
+H = 0.1
+vol = 2.0*L*D*H
+V = 1.5
+R = rho*2*L/(D*H)
+I = V/R
+P = I*V
+Q = P/vol
+Ts = 500
+T(x) = Q*L*L/(2*kappa)*(1-(x/L)*(x/L)) + Ts
+
+
+plot \
+ "$OFDATA" u 1:2 w lines title "OpenFOAM", \
+ T(x) w linespoints lt 0 pt 6 pi 15 title "Analytical"
+EOF
+
+
+echo "End"
+
+#------------------------------------------------------------------------------
diff --git a/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/system/controlDict b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/system/controlDict
new file mode 100644
index 0000000000000000000000000000000000000000..a07195d4fe62c70e9959cc1590c0ebc6fb533317
--- /dev/null
+++ b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/system/controlDict
@@ -0,0 +1,75 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: plus |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application chtMultiRegionSimpleFoam;
+
+startFrom startTime;
+
+startTime 0;
+
+stopAt endTime;
+
+endTime 20000;
+
+deltaT 1;
+
+writeControl timeStep;
+
+writeInterval 50;
+
+purgeWrite 2;
+
+writeFormat ascii;
+
+writePrecision 6;
+
+writeCompression off;
+
+timeFormat general;
+
+timePrecision 6;
+
+runTimeModifiable true;
+
+functions
+{
+ sample1
+ {
+ type sets;
+ libs ("libsampling.so");
+ writeControl outputTime;
+ region solid;
+ fields (T jouleHeatingSource:V jouleHeatingSource:sigma);
+ interpolationScheme cellPoint;
+ setFormat raw;
+
+ sets
+ (
+ centreLine
+ {
+ type uniform;
+ axis x;
+ start (-2.5 0.05 0.05);
+ end ( 2.5 0.05 0.05);
+ nPoints 20;
+ }
+ );
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/system/decomposeParDict b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/system/decomposeParDict
new file mode 100644
index 0000000000000000000000000000000000000000..5448946b393246ebd70ba0b83352f9c4d257c619
--- /dev/null
+++ b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/system/decomposeParDict
@@ -0,0 +1,23 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: plus |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object decomposeParDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains 4;
+
+method scotch;
+
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/system/solid/blockMeshDict b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/system/solid/blockMeshDict
new file mode 100644
index 0000000000000000000000000000000000000000..aad40c34c05f32dc3e2a59a878501abeadb2ef7c
--- /dev/null
+++ b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/system/solid/blockMeshDict
@@ -0,0 +1,89 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: plus |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+convertToMeters 1;
+
+vertices
+(
+ (-2.5 0 0)
+ ( 2.5 0 0)
+ ( 2.5 0.1 0)
+ (-2.5 0.1 0)
+ (-2.5 0 0.1)
+ ( 2.5 0 0.1)
+ ( 2.5 0.1 0.1)
+ (-2.5 0.1 0.1)
+);
+
+blocks
+(
+ hex (0 1 2 3 4 5 6 7) (500 20 1) simpleGrading (1 1 1)
+);
+
+edges
+(
+);
+
+boundary
+(
+ top
+ {
+ type patch;
+ faces
+ (
+ (3 7 6 2)
+ );
+ }
+ bottom
+ {
+ type patch;
+ faces
+ (
+ (1 5 4 0)
+ );
+ }
+ left
+ {
+ type patch;
+ faces
+ (
+ (0 4 7 3)
+ );
+ }
+ right
+ {
+ type patch;
+ faces
+ (
+ (2 6 5 1)
+ );
+ }
+ frontAndBack
+ {
+ type empty;
+ faces
+ (
+ (0 3 2 1)
+ (4 5 6 7)
+ );
+ }
+);
+
+mergePatchPairs
+(
+);
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/system/solid/decomposeParDict b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/system/solid/decomposeParDict
new file mode 120000
index 0000000000000000000000000000000000000000..46638e60f61f453fde97c51772ad6111792db0f6
--- /dev/null
+++ b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/system/solid/decomposeParDict
@@ -0,0 +1 @@
+../decomposeParDict
\ No newline at end of file
diff --git a/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/system/solid/fvOptions b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/system/solid/fvOptions
new file mode 100644
index 0000000000000000000000000000000000000000..114d7e7736edc6ac2c79cda92d90c1c9056b8f98
--- /dev/null
+++ b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/system/solid/fvOptions
@@ -0,0 +1,39 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: plus |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object fvOptions;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+heating
+{
+ type jouleHeatingSource;
+ active true;
+
+ jouleHeatingSourceCoeffs
+ {
+ anisotropicElectricalConductivity no;
+
+ // Optionally specify sigma as a function of temperature
+ //sigma 127599.8469;
+ //
+ //sigma table
+ //(
+ // (0 127599.8469)
+ // (1000 127599.8469)
+ //);
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/system/solid/fvSchemes b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/system/solid/fvSchemes
new file mode 100644
index 0000000000000000000000000000000000000000..3ae1552969519ccbadf1bdce0a105a55cf0db8c8
--- /dev/null
+++ b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/system/solid/fvSchemes
@@ -0,0 +1,50 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: plus |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+ default steadyState;
+}
+
+gradSchemes
+{
+ default Gauss linear;
+}
+
+divSchemes
+{
+ default none;
+}
+
+laplacianSchemes
+{
+ default none;
+ laplacian(alpha,h) Gauss linear uncorrected;
+ laplacian(jouleHeatingSource:sigma,jouleHeatingSource:V) Gauss linear uncorrected;
+}
+
+interpolationSchemes
+{
+ default linear;
+}
+
+snGradSchemes
+{
+ default uncorrected;
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/system/solid/fvSolution b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/system/solid/fvSolution
new file mode 100644
index 0000000000000000000000000000000000000000..b155dcedefa184000b2319c6daf5e5d4abcd398d
--- /dev/null
+++ b/tutorials/heatTransfer/chtMultiRegionSimpleFoam/jouleHeatingSolid/system/solid/fvSolution
@@ -0,0 +1,49 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: plus |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+ h
+ {
+ solver PCG;
+ preconditioner DIC;
+ tolerance 0;
+ relTol 0.1;
+ }
+
+ jouleHeatingSource:V
+ {
+ solver PCG;
+ preconditioner DIC;
+ tolerance 0;
+ relTol 0.1;
+ }
+}
+
+SIMPLE
+{
+ nNonOrthogonalCorrectors 0;
+}
+
+relaxationFactors
+{
+ equations
+ {
+ h 0.99;
+ }
+}
+
+// ************************************************************************* //