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.

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;
+    }
+);
+
+
+// ************************************************************************* //