diff --git a/src/finiteVolume/Make/files b/src/finiteVolume/Make/files
index 783518dfe5..360ecc6b07 100644
--- a/src/finiteVolume/Make/files
+++ b/src/finiteVolume/Make/files
@@ -122,6 +122,7 @@ $(derivedFvPatchFields)/directMappedFixedValue/directMappedFixedValueFvPatchFiel
 $(derivedFvPatchFields)/directMappedVelocityFluxFixedValue/directMappedVelocityFluxFixedValueFvPatchField.C
 $(derivedFvPatchFields)/directMappedFlowRate/directMappedFlowRateFvPatchVectorField.C
 $(derivedFvPatchFields)/fan/fanFvPatchFields.C
+$(derivedFvPatchFields)/fanPressure/fanPressureFvPatchScalarField.C
 $(derivedFvPatchFields)/buoyantPressure/buoyantPressureFvPatchScalarField.C
 $(derivedFvPatchFields)/fixedFluxPressure/fixedFluxPressureFvPatchScalarField.C
 $(derivedFvPatchFields)/fixedInternalValueFvPatchField/fixedInternalValueFvPatchFields.C
diff --git a/src/finiteVolume/fields/fvPatchFields/derived/fanPressure/fanPressureFvPatchScalarField.C b/src/finiteVolume/fields/fvPatchFields/derived/fanPressure/fanPressureFvPatchScalarField.C
new file mode 100644
index 0000000000..db585345f1
--- /dev/null
+++ b/src/finiteVolume/fields/fvPatchFields/derived/fanPressure/fanPressureFvPatchScalarField.C
@@ -0,0 +1,237 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | Copyright (C) 2011-2011 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 "fanPressureFvPatchScalarField.H"
+#include "addToRunTimeSelectionTable.H"
+#include "volFields.H"
+#include "surfaceFields.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+    template<>
+    const char* Foam::NamedEnum
+    <
+        Foam::fanPressureFvPatchScalarField::fanFlowDirection,
+        2
+    >::names[] =
+    {
+        "in",
+        "out"
+    };
+}
+
+const Foam::NamedEnum
+<
+    Foam::fanPressureFvPatchScalarField::fanFlowDirection,
+    2
+> Foam::fanPressureFvPatchScalarField::fanFlowDirectionNames_;
+
+
+// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //
+
+Foam::fanPressureFvPatchScalarField::fanPressureFvPatchScalarField
+(
+    const fvPatch& p,
+    const DimensionedField<scalar, volMesh>& iF
+)
+:
+    fixedValueFvPatchScalarField(p, iF),
+    phiName_("phi"),
+    rhoName_("rho"),
+    p0_(p.size(), 0.0),
+    fanCurve_(),
+    direction_(ffdOut)
+{}
+
+
+Foam::fanPressureFvPatchScalarField::fanPressureFvPatchScalarField
+(
+    const fanPressureFvPatchScalarField& ptf,
+    const fvPatch& p,
+    const DimensionedField<scalar, volMesh>& iF,
+    const fvPatchFieldMapper& mapper
+)
+:
+    fixedValueFvPatchScalarField(ptf, p, iF, mapper),
+    phiName_(ptf.phiName_),
+    rhoName_(ptf.rhoName_),
+    p0_(ptf.p0_, mapper),
+    fanCurve_(ptf.fanCurve_),
+    direction_(ptf.direction_)
+{}
+
+
+Foam::fanPressureFvPatchScalarField::fanPressureFvPatchScalarField
+(
+    const fvPatch& p,
+    const DimensionedField<scalar, volMesh>& iF,
+    const dictionary& dict
+)
+:
+    fixedValueFvPatchScalarField(p, iF),
+    phiName_(dict.lookupOrDefault<word>("phi", "phi")),
+    rhoName_(dict.lookupOrDefault<word>("rho", "rho")),
+    p0_("p0", dict, p.size()),
+    fanCurve_(dict),
+    direction_(fanFlowDirectionNames_.read(dict.lookup("direction")))
+{
+    // Assign initial pressure by "value"
+    fvPatchField<scalar>::operator==(scalarField("value", dict, p.size()));
+}
+
+
+Foam::fanPressureFvPatchScalarField::fanPressureFvPatchScalarField
+(
+    const fanPressureFvPatchScalarField& pfopsf
+)
+:
+    fixedValueFvPatchScalarField(pfopsf),
+    phiName_(pfopsf.phiName_),
+    rhoName_(pfopsf.rhoName_),
+    p0_(pfopsf.p0_),
+    fanCurve_(pfopsf.fanCurve_),
+    direction_(pfopsf.direction_)
+{}
+
+
+Foam::fanPressureFvPatchScalarField::fanPressureFvPatchScalarField
+(
+    const fanPressureFvPatchScalarField& pfopsf,
+    const DimensionedField<scalar, volMesh>& iF
+)
+:
+    fixedValueFvPatchScalarField(pfopsf, iF),
+    phiName_(pfopsf.phiName_),
+    rhoName_(pfopsf.rhoName_),
+    p0_(pfopsf.p0_),
+    fanCurve_(pfopsf.fanCurve_),
+    direction_(pfopsf.direction_)
+{}
+
+
+// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //
+
+void Foam::fanPressureFvPatchScalarField::updateCoeffs()
+{
+    if (updated())
+    {
+        return;
+    }
+
+    // Retrieve flux field
+    const surfaceScalarField& phi =
+        db().lookupObject<surfaceScalarField>(phiName_);
+
+    const fvsPatchField<scalar>& phip =
+        patch().patchField<surfaceScalarField, scalar>(phi);
+
+    int dir = 2*direction_ - 1;
+
+    // Average volumetric flow rate
+    scalar aveFlowRate = 0;
+
+    if (phi.dimensions() == dimVelocity*dimArea)
+    {
+        aveFlowRate = dir*gSum(phip)/gSum(patch().magSf());
+    }
+    else if (phi.dimensions() == dimVelocity*dimArea*dimDensity)
+    {
+        const scalarField& rhop =
+            patch().lookupPatchField<volScalarField, scalar>(rhoName_);
+        aveFlowRate = dir*gSum(phip/rhop)/gSum(patch().magSf());
+    }
+    else
+    {
+        FatalErrorIn("fanPressureFvPatchScalarField::updateCoeffs()")
+            << "dimensions of phi are not correct"
+                << "\n    on patch " << patch().name()
+                << " of field " << dimensionedInternalField().name()
+                << " in file " << dimensionedInternalField().objectPath() << nl
+                << exit(FatalError);
+    }
+
+    // Normal flow through fan
+    if (aveFlowRate >= 0.0)
+    {
+        // Pressure drop for this flow rate
+        const scalar pdFan = fanCurve_(aveFlowRate);
+
+        operator==(p0_ - dir*pdFan);
+    }
+    // Reverse flow
+    else
+    {
+        // Assume that fan has stalled if flow reversed
+        // i.e. apply dp for zero flow rate
+        const scalar pdFan = fanCurve_(0);
+
+        // Flow speed across patch
+        scalarField Up = phip/(patch().magSf());
+
+        // Pressure drop associated withback flow = dynamic pressure
+        scalarField pdBackFlow = 0.5*magSqr(Up);
+
+        if (phi.dimensions() == dimVelocity*dimArea*dimDensity)
+        {
+            const scalarField& rhop =
+                patch().lookupPatchField<volScalarField, scalar>(rhoName_);
+            pdBackFlow /= rhop;
+        }
+
+        operator==(p0_ - dir*(pdBackFlow + pdFan));
+    }
+
+    fixedValueFvPatchScalarField::updateCoeffs();
+}
+
+
+void Foam::fanPressureFvPatchScalarField::write(Ostream& os) const
+{
+    fvPatchScalarField::write(os);
+    os.writeKeyword("phi") << phiName_ << token::END_STATEMENT << nl;
+    os.writeKeyword("rho") << rhoName_ << token::END_STATEMENT << nl;
+    fanCurve_.write(os);
+    os.writeKeyword("direction")
+        << fanFlowDirectionNames_[direction_] << token::END_STATEMENT << nl;
+    p0_.writeEntry("p0", os);
+    writeEntry("value", os);
+}
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+    makePatchTypeField
+    (
+        fvPatchScalarField,
+        fanPressureFvPatchScalarField
+    );
+};
+
+
+// ************************************************************************* //
diff --git a/src/finiteVolume/fields/fvPatchFields/derived/fanPressure/fanPressureFvPatchScalarField.H b/src/finiteVolume/fields/fvPatchFields/derived/fanPressure/fanPressureFvPatchScalarField.H
new file mode 100644
index 0000000000..7c3d9ff411
--- /dev/null
+++ b/src/finiteVolume/fields/fvPatchFields/derived/fanPressure/fanPressureFvPatchScalarField.H
@@ -0,0 +1,205 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     |
+    \\  /    A nd           | Copyright (C) 2011-2011 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::fanPressureFvPatchScalarField
+
+Description
+    Assigns pressure inlet or outlet condition for a fan.
+
+    User specifies:
+    - pressure drop vs volumetric flow rate table (fan curve) file name;
+    - direction of normal flow through the fan, in or out;
+    - total pressure of the environment.
+
+    Example of the boundary condition specification:
+    \verbatim
+        inlet
+        {
+            type            fanPressure;
+            fileName        "fanCurve"; // Fan curve file name
+            outOfBounds     clamp;      // (error|warn|clamp|repeat)
+            direction       in;         // Direction of flow through fan
+            p0              uniform 0;  // Environmental total pressure
+            value           uniform 0;  // Initial pressure
+        }
+
+        outlet
+        {
+            type            fanPressure;
+            fileName        "fanCurve"; // Fan curve file name
+            outOfBounds     clamp;      // (error|warn|clamp|repeat)
+            direction       out;        // Direction of flow through fan
+            p0              uniform 0;  // Environmental total pressure
+            value           uniform 0;  // Initial pressure
+        }
+    \endverbatim
+
+See Also
+    Foam::interpolationTable and
+    Foam::timeVaryingFlowRateInletVelocityFvPatchVectorField
+
+SourceFiles
+    fanPressureFvPatchScalarField.C
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef fanPressureFvPatchScalarField_H
+#define fanPressureFvPatchScalarField_H
+
+#include "fvPatchFields.H"
+#include "fixedValueFvPatchFields.H"
+#include "interpolationTable.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+/*---------------------------------------------------------------------------*\
+              Class fanPressureFvPatchScalarField Declaration
+\*---------------------------------------------------------------------------*/
+
+class fanPressureFvPatchScalarField
+:
+    public fixedValueFvPatchScalarField
+{
+    // Private data
+
+        //- Name of the flux transporting the field
+        word phiName_;
+
+        //- Name of the density field
+        word rhoName_;
+
+        //- Total pressure
+        scalarField p0_;
+
+        //- Tabulated fan curve
+        interpolationTable<scalar> fanCurve_;
+
+        //- Fan flow direction
+        enum fanFlowDirection
+        {
+            ffdIn,
+            ffdOut
+        };
+
+        static const NamedEnum<fanFlowDirection, 2> fanFlowDirectionNames_;
+
+        //- Direction of flow through the fan relative to patch
+        fanFlowDirection direction_;
+
+
+public:
+
+    //- Runtime type information
+    TypeName("fanPressure");
+
+
+    // Constructors
+
+        //- Construct from patch and internal field
+        fanPressureFvPatchScalarField
+        (
+            const fvPatch&,
+            const DimensionedField<scalar, volMesh>&
+        );
+
+        //- Construct from patch, internal field and dictionary
+        fanPressureFvPatchScalarField
+        (
+            const fvPatch&,
+            const DimensionedField<scalar, volMesh>&,
+            const dictionary&
+        );
+
+        //- Construct by mapping given
+        //  fanPressureFvPatchScalarField
+        //  onto a new patch
+        fanPressureFvPatchScalarField
+        (
+            const fanPressureFvPatchScalarField&,
+            const fvPatch&,
+            const DimensionedField<scalar, volMesh>&,
+            const fvPatchFieldMapper&
+        );
+
+        //- Construct as copy
+        fanPressureFvPatchScalarField
+        (
+            const fanPressureFvPatchScalarField&
+        );
+
+        //- Construct and return a clone
+        virtual tmp<fvPatchScalarField> clone() const
+        {
+            return tmp<fvPatchScalarField>
+            (
+                new fanPressureFvPatchScalarField(*this)
+            );
+        }
+
+        //- Construct as copy setting internal field reference
+        fanPressureFvPatchScalarField
+        (
+            const fanPressureFvPatchScalarField&,
+            const DimensionedField<scalar, volMesh>&
+        );
+
+        //- Construct and return a clone setting internal field reference
+        virtual tmp<fvPatchScalarField> clone
+        (
+            const DimensionedField<scalar, volMesh>& iF
+        ) const
+        {
+            return tmp<fvPatchScalarField>
+            (
+                new fanPressureFvPatchScalarField
+                (
+                    *this,
+                    iF
+                )
+            );
+        }
+
+
+    // Member functions
+
+        //- Update the coefficients associated with the patch field
+        virtual void updateCoeffs();
+
+        //- Write
+        virtual void write(Ostream&) const;
+};
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#endif
+
+// ************************************************************************* //