diff --git a/src/finiteVolume/Make/files b/src/finiteVolume/Make/files
index 0fc8dbf70c3fb01ebe2dccb752d356959605024a..2d1b6effb07c56e11d577f8a6dbcad0737b6af23 100644
--- a/src/finiteVolume/Make/files
+++ b/src/finiteVolume/Make/files
@@ -150,6 +150,7 @@ $(derivedFvPatchFields)/turbulentIntensityKineticEnergyInlet/turbulentIntensityK
$(derivedFvPatchFields)/uniformFixedValue/uniformFixedValueFvPatchFields.C
$(derivedFvPatchFields)/waveTransmissive/waveTransmissiveFvPatchFields.C
$(derivedFvPatchFields)/uniformDensityHydrostaticPressure/uniformDensityHydrostaticPressureFvPatchScalarField.C
+$(derivedFvPatchFields)/swirlMassFlowRateInletVelocity/swirlMassFlowRateInletVelocityFvPatchVectorField.C
fvsPatchFields = fields/fvsPatchFields
$(fvsPatchFields)/fvsPatchField/fvsPatchFields.C
diff --git a/src/finiteVolume/fields/fvPatchFields/derived/swirlMassFlowRateInletVelocity/swirlMassFlowRateInletVelocityFvPatchVectorField.C b/src/finiteVolume/fields/fvPatchFields/derived/swirlMassFlowRateInletVelocity/swirlMassFlowRateInletVelocityFvPatchVectorField.C
new file mode 100644
index 0000000000000000000000000000000000000000..c08dbde49564de384d626271b7f76334cebb3965
--- /dev/null
+++ b/src/finiteVolume/fields/fvPatchFields/derived/swirlMassFlowRateInletVelocity/swirlMassFlowRateInletVelocityFvPatchVectorField.C
@@ -0,0 +1,200 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2006-2009 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 2 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, write to the Free Software Foundation,
+ Inc., 51 Franklin St, Fifth Floor, Boston, MA 02110-1301 USA
+
+\*---------------------------------------------------------------------------*/
+
+#include "swirlMassFlowRateInletVelocityFvPatchVectorField.H"
+#include "volFields.H"
+#include "addToRunTimeSelectionTable.H"
+#include "fvPatchFieldMapper.H"
+#include "surfaceFields.H"
+#include "mathematicalConstants.H"
+
+// * * * * * * * * * * * * * * * * Constructors * * * * * * * * * * * * * * //
+
+Foam::
+swirlMassFlowRateInletVelocityFvPatchVectorField::
+swirlMassFlowRateInletVelocityFvPatchVectorField
+(
+ const fvPatch& p,
+ const DimensionedField<vector, volMesh>& iF
+)
+:
+ fixedValueFvPatchField<vector>(p, iF),
+ flowRate_(0),
+ phiName_("phi"),
+ rhoName_("rho"),
+ rpm_(0)
+{}
+
+
+Foam::
+swirlMassFlowRateInletVelocityFvPatchVectorField::
+swirlMassFlowRateInletVelocityFvPatchVectorField
+(
+ const swirlMassFlowRateInletVelocityFvPatchVectorField& ptf,
+ const fvPatch& p,
+ const DimensionedField<vector, volMesh>& iF,
+ const fvPatchFieldMapper& mapper
+)
+:
+ fixedValueFvPatchField<vector>(ptf, p, iF, mapper),
+ flowRate_(ptf.flowRate_),
+ phiName_(ptf.phiName_),
+ rhoName_(ptf.rhoName_)
+{}
+
+
+Foam::
+swirlMassFlowRateInletVelocityFvPatchVectorField::
+swirlMassFlowRateInletVelocityFvPatchVectorField
+(
+ const fvPatch& p,
+ const DimensionedField<vector, volMesh>& iF,
+ const dictionary& dict
+)
+:
+ fixedValueFvPatchField<vector>(p, iF, dict),
+ flowRate_(readScalar(dict.lookup("flowRate"))),
+ phiName_(dict.lookupOrDefault<word>("phi", "phi")),
+ rhoName_(dict.lookupOrDefault<word>("rho", "rho")),
+ rpm_(readScalar(dict.lookup("rpm")))
+{}
+
+
+Foam::
+swirlMassFlowRateInletVelocityFvPatchVectorField::
+swirlMassFlowRateInletVelocityFvPatchVectorField
+(
+ const swirlMassFlowRateInletVelocityFvPatchVectorField& ptf
+)
+:
+ fixedValueFvPatchField<vector>(ptf),
+ flowRate_(ptf.flowRate_),
+ phiName_(ptf.phiName_),
+ rhoName_(ptf.rhoName_),
+ rpm_(ptf.rpm_)
+{}
+
+
+Foam::
+swirlMassFlowRateInletVelocityFvPatchVectorField::
+swirlMassFlowRateInletVelocityFvPatchVectorField
+(
+ const swirlMassFlowRateInletVelocityFvPatchVectorField& ptf,
+ const DimensionedField<vector, volMesh>& iF
+)
+:
+ fixedValueFvPatchField<vector>(ptf, iF),
+ flowRate_(ptf.flowRate_),
+ phiName_(ptf.phiName_),
+ rhoName_(ptf.rhoName_),
+ rpm_(ptf.rpm_)
+{}
+
+
+// * * * * * * * * * * * * * * * Member Functions * * * * * * * * * * * * * //
+
+void Foam::swirlMassFlowRateInletVelocityFvPatchVectorField::updateCoeffs()
+{
+ if (updated())
+ {
+ return;
+ }
+
+ scalar totArea = gSum(patch().magSf());
+ // a simpler way of doing this would be nice
+ scalar avgU = -flowRate_/totArea;
+
+ vector center = gSum(patch().Cf()*patch().magSf())/totArea;
+ vector normal = gSum(patch().nf()*patch().magSf())/totArea;
+
+ vectorField tangVelo =
+ (rpm_*constant::mathematical::pi/30.0)
+ *(patch().Cf() - center) ^ normal;
+
+ vectorField n = patch().nf();
+
+ const surfaceScalarField& phi =
+ db().lookupObject<surfaceScalarField>(phiName_);
+
+ if (phi.dimensions() == dimVelocity*dimArea)
+ {
+ // volumetric flow-rate
+ operator==(tangVelo + n*avgU);
+ }
+ else if (phi.dimensions() == dimDensity*dimVelocity*dimArea)
+ {
+ const fvPatchField<scalar>& rhop =
+ patch().lookupPatchField<volScalarField, scalar>(rhoName_);
+
+ // mass flow-rate
+ operator==(tangVelo + n*avgU/rhop);
+ }
+ else
+ {
+ FatalErrorIn
+ (
+ "swirlMassFlowRateInletVelocityFvPatchVectorField::updateCoeffs()"
+ ) << "dimensions of " << phiName_ << " are incorrect" << nl
+ << " on patch " << this->patch().name()
+ << " of field " << this->dimensionedInternalField().name()
+ << " in file " << this->dimensionedInternalField().objectPath()
+ << nl << exit(FatalError);
+ }
+
+ fixedValueFvPatchField<vector>::updateCoeffs();
+}
+
+
+void Foam::swirlMassFlowRateInletVelocityFvPatchVectorField::write(Ostream& os) const
+{
+ fvPatchField<vector>::write(os);
+ os.writeKeyword("flowRate") << flowRate_ << token::END_STATEMENT << nl;
+ if (phiName_ != "phi")
+ {
+ os.writeKeyword("phi") << phiName_ << token::END_STATEMENT << nl;
+ }
+ if (rhoName_ != "rho")
+ {
+ os.writeKeyword("rho") << rhoName_ << token::END_STATEMENT << nl;
+ }
+ os.writeKeyword("rpm") << rpm_ << token::END_STATEMENT << nl;
+ writeEntry("value", os);
+}
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+ makePatchTypeField
+ (
+ fvPatchVectorField,
+ swirlMassFlowRateInletVelocityFvPatchVectorField
+ );
+}
+
+
+// ************************************************************************* //
diff --git a/src/finiteVolume/fields/fvPatchFields/derived/swirlMassFlowRateInletVelocity/swirlMassFlowRateInletVelocityFvPatchVectorField.H b/src/finiteVolume/fields/fvPatchFields/derived/swirlMassFlowRateInletVelocity/swirlMassFlowRateInletVelocityFvPatchVectorField.H
new file mode 100644
index 0000000000000000000000000000000000000000..bef41d4655cc95eb07a3f875721803e2cf4450eb
--- /dev/null
+++ b/src/finiteVolume/fields/fvPatchFields/derived/swirlMassFlowRateInletVelocity/swirlMassFlowRateInletVelocityFvPatchVectorField.H
@@ -0,0 +1,191 @@
+/*---------------------------------------------------------------------------*\
+ ========= |
+ \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
+ \\ / O peration |
+ \\ / A nd | Copyright (C) 2010-2010 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 2 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, write to the Free Software Foundation,
+ Inc., 51 Franklin St, Fifth Floor, Boston, MA 02110-1301 USA
+
+Class
+ Foam::swirlMassFlowRateInletVelocityFvPatchVectorField
+
+Description
+ Describes a volumetric/mass flow normal vector boundary condition by its
+ magnitude as an integral over its area with a swirl component determined
+ by the RPM
+
+ The basis of the patch (volumetric or mass) is determined by the
+ dimensions of the flux, phi.
+ The current density is used to correct the velocity when applying the
+ mass basis.
+
+ Example of the boundary condition specification:
+ @verbatim
+ inlet
+ {
+ type swirlMassFlowRateInletVelocity;
+ flowRate 0.2; // Volumetric/mass flow rate [m3/s or kg/s]
+ rpm 100;
+ }
+ @endverbatim
+
+Note
+ - The value is positive inwards
+
+SourceFiles
+ swirlMassFlowRateInletVelocityFvPatchVectorField.C
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef swirlMassFlowRateInletVelocityFvPatchVectorField_H
+#define swirlMassFlowRateInletVelocityFvPatchVectorField_H
+
+#include "fixedValueFvPatchFields.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+/*---------------------------------------------------------------------------*\
+ Class swirlMassFlowRateInletVelocityFvPatchVectorField Declaration
+\*---------------------------------------------------------------------------*/
+
+class swirlMassFlowRateInletVelocityFvPatchVectorField
+:
+ public fixedValueFvPatchVectorField
+{
+ // Private data
+
+ //- Inlet integral flow rate
+ scalar flowRate_;
+
+ //- Name of the flux transporting the field
+ word phiName_;
+
+ //- Name of the density field used to normalize the mass flux
+ word rhoName_;
+
+ //- RPM
+ scalar rpm_;
+
+
+public:
+
+ //- Runtime type information
+ TypeName("swirlMassFlowRateInletVelocity");
+
+
+ // Constructors
+
+ //- Construct from patch and internal field
+ swirlMassFlowRateInletVelocityFvPatchVectorField
+ (
+ const fvPatch&,
+ const DimensionedField<vector, volMesh>&
+ );
+
+ //- Construct from patch, internal field and dictionary
+ swirlMassFlowRateInletVelocityFvPatchVectorField
+ (
+ const fvPatch&,
+ const DimensionedField<vector, volMesh>&,
+ const dictionary&
+ );
+
+ //- Construct by mapping given
+ // flowRateInletVelocityFvPatchVectorField
+ // onto a new patch
+ swirlMassFlowRateInletVelocityFvPatchVectorField
+ (
+ const swirlMassFlowRateInletVelocityFvPatchVectorField&,
+ const fvPatch&,
+ const DimensionedField<vector, volMesh>&,
+ const fvPatchFieldMapper&
+ );
+
+ //- Construct as copy
+ swirlMassFlowRateInletVelocityFvPatchVectorField
+ (
+ const swirlMassFlowRateInletVelocityFvPatchVectorField&
+ );
+
+ //- Construct and return a clone
+ virtual tmp<fvPatchVectorField> clone() const
+ {
+ return tmp<fvPatchVectorField>
+ (
+ new swirlMassFlowRateInletVelocityFvPatchVectorField(*this)
+ );
+ }
+
+ //- Construct as copy setting internal field reference
+ swirlMassFlowRateInletVelocityFvPatchVectorField
+ (
+ const swirlMassFlowRateInletVelocityFvPatchVectorField&,
+ const DimensionedField<vector, volMesh>&
+ );
+
+ //- Construct and return a clone setting internal field reference
+ virtual tmp<fvPatchVectorField> clone
+ (
+ const DimensionedField<vector, volMesh>& iF
+ ) const
+ {
+ return tmp<fvPatchVectorField>
+ (
+ new swirlMassFlowRateInletVelocityFvPatchVectorField(*this, iF)
+ );
+ }
+
+
+ // Member functions
+
+ // Access
+
+ //- Return the flux
+ scalar flowRate() const
+ {
+ return flowRate_;
+ }
+
+ //- Return reference to the flux to allow adjustment
+ scalar& flowRate()
+ {
+ return flowRate_;
+ }
+
+
+ //- Update the coefficients associated with the patch field
+ virtual void updateCoeffs();
+
+ //- Write
+ virtual void write(Ostream&) const;
+
+};
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //