prghCyclicPressure: New cyclic boundary condition for p_rgh

This boundary condition provides a cyclic condition for p_rgh. It applies
corrections to the value and gradient on both sides of the cyclic to
account for the non-cylicity of the gravitational force.

This condition is only needed when the cyclic patches have a transformation
and a normal component in the direction of gravity. If the cyclic patches
are orthogonal to the direction gravity, then a normal cyclic boundary
condition can be used instead.

Care must be taken when using this boundary condition that the simulation
is actually cyclic. The following constraints apply:

- Both cyclic patches must be oriented in the same way with respect to
  gravity. In practice this means that applicability is limited to cyclics
  with translational transformations.

- The model cannot have any dependence on the absolute value of the
  pressure field. The absolute value of the pressure, in reality, varies
  between each repetition of the geometry; it is not actually formally
  cyclic. Only the gradient of the pressure field can be truly cyclic. This
  model is therefore only valid if the absolute value of the pressure is
  arbitrary, and only the gradient has an effect on the solution. This is
  the case for incompressible multiphase solutions or incompressible
  Boussinesq-like models of density variation. It is not true if (for
  example) a compressible thermodynamic model is being used.

Specification is as follows. A "patchType" entry must be provided to
indicate that this condition overrides the underlying cyclic constraint,
and a "rhoInf" entry is needed (by the owner patch only) to specify the
density of the far-field environment. For example:

    cyclicA
    {
        type            prghCyclicPressure;
        patchType       cyclic;
        rhoInf          1; // [kg/m^3]
    }

    cyclicB
    {
        type            prghCyclicPressure;
        patchType       cyclic;
    }

A tutorial, incompressibleVoF/trayedPipe, has been added to demonstrate
usage of this boundary condition.

src/finiteVolume/Make/files

@@ -257,6 +257,7 @@ $(derivedFvPatchFields)/PrghPressure/prghPressureFvPatchScalarFields.C
 $(derivedFvPatchFields)/prghTotalHydrostaticPressure/prghTotalHydrostaticPressureFvPatchScalarField.C
 $(derivedFvPatchFields)/fixedValueInletOutlet/fixedValueInletOutletFvPatchFields.C
 $(derivedFvPatchFields)/transonicEntrainmentPressure/transonicEntrainmentPressureFvPatchScalarField.C
+$(derivedFvPatchFields)/prghCyclicPressure/prghCyclicPressureFvPatchScalarField.C
 
 fvsPatchFields = fields/fvsPatchFields
 $(fvsPatchFields)/fvsPatchField/fvsPatchFields.C

src/finiteVolume/fields/fvPatchFields/derived/prghCyclicPressure/prghCyclicPressureFvPatchScalarField.C

@@ -0,0 +1,207 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Copyright (C) 2024 OpenFOAM Foundation
+     \\/     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 "prghCyclicPressureFvPatchScalarField.H"
+#include "addToRunTimeSelectionTable.H"
+#include "fieldMapper.H"
+#include "volFields.H"
+#include "surfaceFields.H"
+#include "fvcSnGrad.H"
+
+// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //
+
+Foam::prghCyclicPressureFvPatchScalarField::prghCyclicPressureFvPatchScalarField
+(
+    const fvPatch& p,
+    const DimensionedField<scalar, volMesh>& iF,
+    const dictionary& dict
+)
+:
+    jumpCyclicFvPatchScalarField(p, iF, dict),
+    rhoName_
+    (
+        cyclicPatch().owner()
+      ? dict.lookupOrDefault<word>("rho", "rho")
+      : word::null
+    ),
+    rhoInf_(cyclicPatch().owner() ? dict.lookup<scalar>("rhoInf") : NaN),
+    jump_(p.size(), Zero)
+{
+    if (dict.found("jump"))
+    {
+        jump_ = scalarField("jump", dict, p.size());
+    }
+
+    evaluateNoUpdateCoeffs();
+}
+
+
+Foam::prghCyclicPressureFvPatchScalarField::prghCyclicPressureFvPatchScalarField
+(
+    const prghCyclicPressureFvPatchScalarField& ptf,
+    const fvPatch& p,
+    const DimensionedField<scalar, volMesh>& iF,
+    const fieldMapper& mapper
+)
+:
+    jumpCyclicFvPatchScalarField(ptf, p, iF, mapper),
+    rhoName_(ptf.rhoName_),
+    rhoInf_(ptf.rhoInf_),
+    jump_(mapper(ptf.jump_))
+{}
+
+
+Foam::prghCyclicPressureFvPatchScalarField::prghCyclicPressureFvPatchScalarField
+(
+    const prghCyclicPressureFvPatchScalarField& ptf,
+    const DimensionedField<scalar, volMesh>& iF
+)
+:
+    jumpCyclicFvPatchScalarField(ptf, iF),
+    rhoName_(ptf.rhoName_),
+    rhoInf_(ptf.rhoInf_),
+    jump_(ptf.jump_)
+{}
+
+
+// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //
+
+Foam::tmp<Foam::scalarField>
+Foam::prghCyclicPressureFvPatchScalarField::jump() const
+{
+    return jump_;
+}
+
+
+void Foam::prghCyclicPressureFvPatchScalarField::map
+(
+    const fvPatchScalarField& ptf,
+    const fieldMapper& mapper
+)
+{
+    jumpCyclicFvPatchScalarField::map(ptf, mapper);
+
+    const prghCyclicPressureFvPatchScalarField& tiptf =
+        refCast<const prghCyclicPressureFvPatchScalarField>(ptf);
+
+    mapper(jump_, tiptf.jump_);
+}
+
+
+void Foam::prghCyclicPressureFvPatchScalarField::reset
+(
+    const fvPatchScalarField& ptf
+)
+{
+    jumpCyclicFvPatchScalarField::reset(ptf);
+
+    const prghCyclicPressureFvPatchScalarField& tiptf =
+        refCast<const prghCyclicPressureFvPatchScalarField>(ptf);
+
+    jump_.reset(tiptf.jump_);
+}
+
+
+void Foam::prghCyclicPressureFvPatchScalarField::updateCoeffs()
+{
+    if (updated())
+    {
+        return;
+    }
+
+    const volScalarField& vf =
+        static_cast<const volScalarField&>(internalField());
+
+    const prghCyclicPressureFvPatchScalarField& nbrPf =
+        refCast<const prghCyclicPressureFvPatchScalarField>(nbrPatchField());
+
+    const label patchi = patch().index(), nbrPatchi = nbrPf.patch().index();
+
+    // Buoyancy fields
+    const volScalarField& rhoVf =
+        db().lookupObject<volScalarField>
+        (cyclicPatch().owner() ? rhoName_ : nbrPf.rhoName_);
+    const volScalarField::Boundary& rhoBf = rhoVf.boundaryField();
+    const surfaceScalarField::Boundary& ghfBf =
+        db().lookupObject<surfaceScalarField>("ghf").boundaryField();
+
+    // Pressure solution fields
+    const surfaceScalarField::Boundary& rAUfBf =
+        db().lookupObject<surfaceScalarField>("rAUf").boundaryField();
+    const surfaceScalarField::Boundary& phiHbyABf =
+        db().lookupObject<surfaceScalarField>("phiHbyA").boundaryField();
+
+    // Delta coefficients for this field
+    const tmp<surfaceScalarField> deltaCoeffsSf =
+        fv::snGradScheme<scalar>::New
+        (
+            vf.mesh(),
+            vf.mesh().schemes().snGrad(internalField().name())
+        )->deltaCoeffs(vf);
+    const scalarField& deltaCoeffsPf =
+        deltaCoeffsSf->boundaryField()[patch().index()];
+
+    // Calculate the jump
+    jump_ =
+        (rhoBf[patchi] - (cyclicPatch().owner() ? rhoInf_ : nbrPf.rhoInf_))
+       *(ghfBf[nbrPatchi] - ghfBf[patchi])
+      + (
+            phiHbyABf[patchi]/rAUfBf[patchi]/patch().magSf()
+          + phiHbyABf[nbrPatchi]/rAUfBf[nbrPatchi]/nbrPf.patch().magSf()
+        )*patch().weights()/deltaCoeffsPf;
+
+    jumpCyclicFvPatchScalarField::updateCoeffs();
+}
+
+
+void Foam::prghCyclicPressureFvPatchScalarField::write
+(
+    Ostream& os
+) const
+{
+    fvPatchScalarField::write(os);
+
+    if (cyclicPatch().owner())
+    {
+        writeEntryIfDifferent<word>(os, "rho", "rho", rhoName_);
+        writeEntry(os, "rhoInf", rhoInf_);
+    }
+
+    writeEntry(os, "jump", jump_);
+}
+
+
+// * * * * * * * * * * * * * * Build Macro Function  * * * * * * * * * * * * //
+
+namespace Foam
+{
+    makePatchTypeField
+    (
+        fvPatchScalarField,
+        prghCyclicPressureFvPatchScalarField
+    );
+}
+
+// ************************************************************************* //

src/finiteVolume/fields/fvPatchFields/derived/prghCyclicPressure/prghCyclicPressureFvPatchScalarField.H

@@ -0,0 +1,217 @@
+/*---------------------------------------------------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Copyright (C) 2024 OpenFOAM Foundation
+     \\/     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::prghCyclicPressureFvPatchScalarField
+
+Description
+    This boundary condition provides a cyclic condition for p_rgh. It applies
+    corrections to the value and gradient on both sides of the cyclic to
+    account for the non-cylicity of the gravitational force.
+
+    This condition is only needed when the cyclic patches have a transformation
+    and a normal component in the direction of gravity. If the cyclic patches
+    are orthogonal to the direction gravity, then a normal cyclic boundary
+    condition can be used instead.
+
+    Care must be taken when using this boundary condition that the simulation
+    is actually cyclic. The following constraints apply:
+
+    - Both cyclic patches must be oriented in the same way with respect to
+      gravity. In practice this means that applicability is limited to cyclics
+      with translational transformations.
+
+    - The model cannot have any dependence on the absolute value of the
+      pressure field. The absolute value of the pressure, in reality, varies
+      between each repetition of the geometry; it is not actually formally
+      cyclic. Only the gradient of the pressure field can be truly cyclic. This
+      model is therefore only valid if the absolute value of the pressure is
+      arbitrary, and only the gradient has an effect on the solution. This is
+      the case for incompressible multiphase solutions or incompressible
+      Boussinesq-like models of density variation. It is not true if (for
+      example) a compressible thermodynamic model is being used.
+
+Usage
+    \table
+        Property     | Description             | Required    | Default value
+        patchType    | underlying patch type (should be \c cyclic) | yes |
+        rhoInf       | far-field density       | yes         |
+    \endtable
+
+    Example of the boundary condition specification:
+    \verbatim
+    <patchName>
+    {
+        type            prghCyclicPressure;
+        patchType       cyclic;
+        rhoInf          1;
+    }
+    \endverbatim
+
+SourceFiles
+    prghCyclicPressureFvPatchScalarField.C
+
+\*---------------------------------------------------------------------------*/
+
+#ifndef prghCyclicPressureFvPatchScalarField_H
+#define prghCyclicPressureFvPatchScalarField_H
+
+#include "jumpCyclicFvPatchFields.H"
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+namespace Foam
+{
+
+/*---------------------------------------------------------------------------*\
+            Class prghCyclicPressureFvPatchScalarField Declaration
+\*---------------------------------------------------------------------------*/
+
+class prghCyclicPressureFvPatchScalarField
+:
+    public jumpCyclicFvPatchScalarField
+{
+    // Private Data
+
+        //- Name of the density field
+        const word rhoName_;
+
+        //- Far-field density
+        const scalar rhoInf_;
+
+        //- Jump in value from the other patch to this one
+        scalarField jump_;
+
+
+    // Private Member Functions
+
+        //- Get the far-field density from the owner patch
+        scalar rhoInf() const;
+
+        //- Update result field based on interface functionality
+        template<class ... Cmpt>
+        void updateInterfaceMatrix
+        (
+            scalarField& result,
+            const scalarField& psiInternal,
+            const scalarField& coeffs,
+            const Pstream::commsTypes commsType,
+            const Cmpt ... cmpt
+        ) const;
+
+
+public:
+
+    //- Runtime type information
+    TypeName("prghCyclicPressure");
+
+
+    // Constructors
+
+        //- Construct from patch, internal field and dictionary
+        prghCyclicPressureFvPatchScalarField
+        (
+            const fvPatch&,
+            const DimensionedField<scalar, volMesh>&,
+            const dictionary&
+        );
+
+        //- Construct by mapping given fixedValueTypeFvPatchField
+        //  onto a new patch
+        prghCyclicPressureFvPatchScalarField
+        (
+            const prghCyclicPressureFvPatchScalarField&,
+            const fvPatch&,
+            const DimensionedField<scalar, volMesh>&,
+            const fieldMapper&
+        );
+
+        //- Disallow copy without setting internal field reference
+        prghCyclicPressureFvPatchScalarField
+        (
+            const prghCyclicPressureFvPatchScalarField&
+        ) = delete;
+
+        //- Copy constructor setting internal field reference
+        prghCyclicPressureFvPatchScalarField
+        (
+            const prghCyclicPressureFvPatchScalarField&,
+            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 prghCyclicPressureFvPatchScalarField
+                (
+                    *this,
+                    iF
+                )
+            );
+        }
+
+
+    // Member Functions
+
+        // Access
+
+            //- Return the "jump"
+            virtual tmp<scalarField> jump() const;
+
+
+        // Mapping functions
+
+            //- Map the given fvPatchField onto this fvPatchField
+            virtual void map(const fvPatchScalarField&, const fieldMapper&);
+
+            //- Reset the fvPatchField to the given fvPatchField
+            //  Used for mesh to mesh mapping
+            virtual void reset(const fvPatchScalarField&);
+
+
+        // Evaluation functions
+
+            //- Update the patch pressure gradient field
+            virtual void updateCoeffs();
+
+
+        //- Write
+        virtual void write(Ostream&) const;
+};
+
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+} // End namespace Foam
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+
+#endif
+
+// ************************************************************************* //

tutorials/incompressibleVoF/trayedPipe/0/U

@@ -0,0 +1,32 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       volVectorField;
+    location    "0";
+    object      U;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 1 -1 0 0 0 0];
+
+internalField   uniform (0 0 0);
+
+boundaryField
+{
+    #includeEtc "caseDicts/setConstraintTypes"
+
+    wall
+    {
+        type            noSlip;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/incompressibleVoF/trayedPipe/0/alpha.water.orig

@@ -0,0 +1,32 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       volScalarField;
+    location    "0";
+    object      alpha.water;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    #includeEtc "caseDicts/setConstraintTypes"
+
+    wall
+    {
+        type            zeroGradient;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/incompressibleVoF/trayedPipe/0/p_rgh

@@ -0,0 +1,44 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       volScalarField;
+    location    "0";
+    object      p_rgh;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [1 -1 -2 0 0 0 0];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    #includeEtc "caseDicts/setConstraintTypes"
+
+    wall
+    {
+        type            fixedFluxPressure;
+        value           $internalField;
+    }
+    bottom
+    {
+        type            prghCyclicPressure;
+        patchType       cyclic;
+        rhoInf          1;
+    }
+    top
+    {
+        type            prghCyclicPressure;
+        patchType       cyclic;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/incompressibleVoF/trayedPipe/Allclean

@@ -0,0 +1,9 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # Run from this directory
+
+# Source tutorial clean functions
+. $WM_PROJECT_DIR/bin/tools/CleanFunctions
+
+cleanVoFCase
+
+#------------------------------------------------------------------------------

tutorials/incompressibleVoF/trayedPipe/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
+
+runApplication blockMesh
+runApplication topoSet
+runApplication createBaffles -overwrite
+runApplication setFields
+runApplication $(getApplication)
+
+#------------------------------------------------------------------------------

tutorials/incompressibleVoF/trayedPipe/constant/g

@@ -0,0 +1,21 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       uniformDimensionedVectorField;
+    location    "constant";
+    object      g;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 1 -2 0 0 0 0];
+value           (0 -9.81 0);
+
+
+// ************************************************************************* //

tutorials/incompressibleVoF/trayedPipe/constant/hRef

@@ -0,0 +1,23 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       uniformDimensionedScalarField;
+    location    "constant";
+    object      hRef;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#include "$FOAM_CASE/system/blockMeshDict"
+
+dimensions      [0 1 0 0 0 0 0];
+value           #calc "$<scalar>{height}/2";
+
+
+// ************************************************************************* //

tutorials/incompressibleVoF/trayedPipe/constant/momentumTransport

@@ -0,0 +1,20 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      momentumTransport;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType  laminar;
+
+
+// ************************************************************************* //

tutorials/incompressibleVoF/trayedPipe/constant/phaseProperties

@@ -0,0 +1,22 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      phaseProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+phases          (water air);
+
+sigma           0.07;
+
+
+// ************************************************************************* //

tutorials/incompressibleVoF/trayedPipe/constant/physicalProperties.air

@@ -0,0 +1,24 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      physicalProperties.air;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+viscosityModel  constant;
+
+nu              1.48e-05;
+
+rho             1;
+
+
+// ************************************************************************* //

tutorials/incompressibleVoF/trayedPipe/constant/physicalProperties.water

@@ -0,0 +1,24 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      physicalProperties.water;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+viscosityModel  constant;
+
+nu              1e-06;
+
+rho             1000;
+
+
+// ************************************************************************* //

tutorials/incompressibleVoF/trayedPipe/system/blockMeshDict

@@ -0,0 +1,89 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+height          0.045;
+radius          0.015;
+nCellsPerMetre  2666.67;
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+halfThickness #calc "scalar(1)/$<scalar>nCellsPerMetre";
+
+nCellsHeight #calc "round($<scalar>height*$<scalar>nCellsPerMetre)";
+nCellsRadius #calc "round($<scalar>radius*$<scalar>nCellsPerMetre)";
+
+convertToMeters 1;
+
+vertices
+(
+    (0 0 0) (0 $height 0)
+    ($radius 0 #neg $halfThickness) ($radius $height #neg $halfThickness)
+    ($radius 0 $halfThickness) ($radius $height $halfThickness)
+);
+
+blocks
+(
+    hex (1 0 2 3 1 0 4 5) ($nCellsHeight $nCellsRadius 1) simpleGrading (1 1 1)
+);
+
+boundary
+(
+    walls
+    {
+        type wall;
+        faces
+        (
+            (2 3 5 4)
+        );
+    }
+    bottom
+    {
+        type cyclic;
+        faces
+        (
+            (0 0 2 4)
+        );
+        neighbourPatch top;
+    }
+    top
+    {
+        type cyclic;
+        faces
+        (
+            (1 1 3 5)
+        );
+        neighbourPatch bottom;
+    }
+    wedgeBack
+    {
+        type wedge;
+        faces
+        (
+            (0 1 3 2)
+        );
+    }
+    wedgeFront
+    {
+        type wedge;
+        faces
+        (
+            (0 1 5 4)
+        );
+    }
+);
+
+
+// ************************************************************************* //

tutorials/incompressibleVoF/trayedPipe/system/controlDict

@@ -0,0 +1,57 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application     foamRun;
+
+solver          incompressibleVoF;
+
+startFrom       startTime;
+
+startTime       0;
+
+stopAt          endTime;
+
+endTime         2;
+
+deltaT          0.0001;
+
+writeControl    adjustableRunTime;
+
+writeInterval   0.005;
+
+purgeWrite      0;
+
+writeFormat     binary;
+
+writePrecision  6;
+
+writeCompression off;
+
+timeFormat      general;
+
+timePrecision   6;
+
+runTimeModifiable yes;
+
+adjustTimeStep  yes;
+
+maxCo           1;
+maxAlphaCo      1;
+
+maxDeltaT       1;
+
+
+// ************************************************************************* //

tutorials/incompressibleVoF/trayedPipe/system/createBafflesDict

@@ -0,0 +1,39 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      createBafflesDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+internalFacesOnly true;
+
+baffles
+{
+    wall
+    {
+        type        faceZone;
+        zoneName    baffles;
+
+        owner
+        {
+            name        baffles;
+            type        wall;
+        }
+        neighbour
+        {
+            $owner;
+        }
+    }
+}
+
+
+// ************************************************************************* //

tutorials/incompressibleVoF/trayedPipe/system/fvSchemes

@@ -0,0 +1,50 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+    default         Euler;
+}
+
+gradSchemes
+{
+    default         Gauss linear;
+}
+
+divSchemes
+{
+    div(phi,alpha)  Gauss interfaceCompression vanLeer 1;
+    div(rhoPhi,U)   Gauss linearUpwind grad(U);
+    div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
+}
+
+laplacianSchemes
+{
+    default         Gauss linear uncorrected;
+}
+
+interpolationSchemes
+{
+    default         linear;
+}
+
+snGradSchemes
+{
+    default         uncorrected;
+}
+
+
+// ************************************************************************* //

tutorials/incompressibleVoF/trayedPipe/system/fvSolution

@@ -0,0 +1,74 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+    "alpha.water.*"
+    {
+        nAlphaCorr      2;
+        nAlphaSubCycles 1;
+
+        MULESCorr       yes;
+        nLimiterIter    3;
+
+        solver          smoothSolver;
+        smoother        symGaussSeidel;
+        tolerance       1e-8;
+        relTol          0;
+    }
+
+    "pcorr.*"
+    {
+        solver          PCG;
+        preconditioner  DIC;
+        tolerance       1e-5;
+        relTol          0;
+    }
+
+    p_rgh
+    {
+        $pcorr;
+        tolerance       1e-7;
+        relTol          0.05;
+    }
+
+    p_rghFinal
+    {
+        $p_rgh;
+        relTol          0;
+    }
+}
+
+PIMPLE
+{
+    momentumPredictor   no;
+    nOuterCorrectors    1;
+    nCorrectors         3;
+    nNonOrthogonalCorrectors 0;
+    pRefPoint           (0 0.015 0);
+    pRefValue           0;
+}
+
+relaxationFactors
+{
+    equations
+    {
+        ".*"                1;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/incompressibleVoF/trayedPipe/system/setFieldsDict

@@ -0,0 +1,43 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      setFieldsDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+alphaMean       0.25;
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#include "blockMeshDict"
+
+defaultFieldValues
+(
+    volScalarFieldValue alpha.water 0
+);
+
+regions
+(
+    cylinderToCell
+    {
+        point1  (0 0 0);
+        point2  (0 $height 0);
+        radius  #calc "$<scalar>radius*sqrt($<scalar>alphaMean)";
+        fieldValues
+        (
+            volScalarFieldValue alpha.water 1
+        );
+    }
+);
+
+
+// ************************************************************************* //

tutorials/incompressibleVoF/trayedPipe/system/topoSetDict

@@ -0,0 +1,128 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      topoSetDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+nBaffles        6;
+baffleOverlap   0.4;
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#include "blockMeshDict"
+
+innerBaffleOuterRadius #calc "$<scalar>{radius}/(2 - $<scalar>baffleOverlap)";
+outerBaffleInnerRadius #calc "$radius - $innerBaffleOuterRadius";
+
+actions
+(
+    // Create baffles along the length of the pipe, alternating the zone
+    // between "innerBaffles" and "outerBaffles"
+    #codeStream
+    {
+        code
+        #{
+            for (label i = 0; i < $<label>nBaffles; ++ i)
+            {
+                const scalar y =
+                    scalar(2*i + 1)/(2*$<label>nBaffles)*$<scalar>height;
+
+                os <<
+                    dictionary
+                    (
+                        "action", i<2 ? "new" : "add",
+                        "type", "faceZoneSet",
+                        "name", word(i%2 ? "inner" : "outer") + "Baffles",
+                        "source", "planeToFaceZone",
+                        "point", vector(0, y, 0),
+                        "normal", vector(0, 1, 0)
+                    );
+            }
+        #};
+    }
+
+    // Cut away the outer portion of the inner baffles
+    {
+        action  new;
+        type    faceSet;
+        name    innerBaffles;
+        source  zoneToFace;
+        zone    innerBaffles;
+    }
+    {
+        action  delete;
+        type    faceSet;
+        name    innerBaffles;
+        source  cylinderAnnulusToFace;
+        point1  (0 0 0);
+        point2  (0 $height 0);
+        innerRadius $innerBaffleOuterRadius;
+        outerRadius $radius;
+    }
+
+    // Cut away the inner portion of the outer baffles
+    {
+        action  new;
+        type    faceSet;
+        name    outerBaffles;
+        source  zoneToFace;
+        zone    outerBaffles;
+    }
+    {
+        action  delete;
+        type    faceSet;
+        name    outerBaffles;
+        source  cylinderToFace;
+        point1  (0 0 0);
+        point2  (0 $height 0);
+        radius  $outerBaffleInnerRadius;
+    }
+
+    // Combine inner and outer baffles into a single zone
+    {
+        action  new;
+        type    faceZoneSet;
+        name    baffles;
+        source  setAndNormalToFaceZone;
+        set     innerBaffles;
+        normal  (0 1 0);
+    }
+    {
+        action  add;
+        type    faceZoneSet;
+        name    baffles;
+        source  setAndNormalToFaceZone;
+        set     outerBaffles;
+        normal  (0 1 0);
+    }
+
+    // Clean up
+    {
+        action  remove;
+        type    faceSet;
+        name    innerBaffles;
+    }
+    {
+        action  remove;
+        type    faceSet;
+        name    outerBaffles;
+    }
+    {
+        action  remove;
+        type    faceSet;
+        name    baffles;
+    }
+);
+
+
+// ************************************************************************* //