diff --git a/tutorials/multiphase/interIsoFoam/iobasin/0.orig/U b/tutorials/multiphase/interIsoFoam/iobasin/0.orig/U
new file mode 100644
index 0000000000000000000000000000000000000000..fcc166b1155cfec6a46dd51e1270a2a53db8be0d
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/iobasin/0.orig/U
@@ -0,0 +1,49 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volVectorField;
+ object U;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 1 -1 0 0 0 0];
+
+internalField uniform (0.1 0 0);
+
+boundaryField
+{
+ inlet
+ {
+ type flowRateInletVelocity;
+ volumetricFlowRate constant 0.1;
+ }
+
+ walls
+ {
+ type slip;
+ }
+
+ outlet
+ {
+ type flowRateOutletVelocity;
+ volumetricFlowRate constant 0.1;
+ }
+
+ atmosphere
+ {
+ type pressureInletOutletVelocity;
+ value uniform (0 0 0);
+ }
+
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/iobasin/0.orig/alpha.water b/tutorials/multiphase/interIsoFoam/iobasin/0.orig/alpha.water
new file mode 100644
index 0000000000000000000000000000000000000000..7c8c91473292175b98c98f5a2453b5c210f39e06
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/iobasin/0.orig/alpha.water
@@ -0,0 +1,48 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ object alpha.water;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 0 0 0 0 0 0];
+
+internalField uniform 0;
+
+boundaryField
+{
+ inlet
+ {
+ type fixedValue;
+ value uniform 1;
+ }
+
+ walls
+ {
+ type zeroGradient;
+ }
+
+ outlet
+ {
+ type zeroGradient;
+ value uniform 0;
+ }
+
+ atmosphere
+ {
+ type inletOutlet;
+ inletValue uniform 0;
+ value uniform 0;
+ }
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/iobasin/0.orig/p_rgh b/tutorials/multiphase/interIsoFoam/iobasin/0.orig/p_rgh
new file mode 100644
index 0000000000000000000000000000000000000000..3867a5548344b4d26ebda557ee7093587e7945a7
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/iobasin/0.orig/p_rgh
@@ -0,0 +1,47 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ object p_rgh;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [1 -1 -2 0 0 0 0];
+
+internalField uniform 0;
+
+boundaryField
+{
+ inlet
+ {
+ type zeroGradient;
+ }
+
+ walls
+ {
+ type fixedFluxPressure;
+ value uniform 0;
+ }
+
+ outlet
+ {
+ type zeroGradient;
+ }
+
+ atmosphere
+ {
+ type totalPressure;
+ p0 uniform 0;
+ }
+
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/iobasin/Allclean b/tutorials/multiphase/interIsoFoam/iobasin/Allclean
new file mode 100755
index 0000000000000000000000000000000000000000..e2f275d9fd6e6ba843f14fec57e2987e4c8607b3
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/iobasin/Allclean
@@ -0,0 +1,7 @@
+#!/bin/sh
+cd ${0%/*} || exit 1 # Run from this directory
+. $WM_PROJECT_DIR/bin/tools/CleanFunctions # Tutorial clean functions
+
+cleanCase0
+
+#------------------------------------------------------------------------------
diff --git a/tutorials/multiphase/interIsoFoam/iobasin/Allrun b/tutorials/multiphase/interIsoFoam/iobasin/Allrun
new file mode 100755
index 0000000000000000000000000000000000000000..90ac4929521659a246995e14b41521f49729d13f
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/iobasin/Allrun
@@ -0,0 +1,12 @@
+#!/bin/sh
+cd ${0%/*} || exit 1 # Run from this directory
+. $WM_PROJECT_DIR/bin/tools/RunFunctions # Tutorial run functions
+
+restore0Dir
+runApplication blockMesh
+runApplication createPatch -overwrite
+runApplication setFields
+runApplication decomposePar
+runParallel $(getApplication)
+
+#------------------------------------------------------------------------------
diff --git a/tutorials/multiphase/interIsoFoam/iobasin/constant/g b/tutorials/multiphase/interIsoFoam/iobasin/constant/g
new file mode 100644
index 0000000000000000000000000000000000000000..bded3688c0600a4e15e99a23892da0fb60d689e2
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/iobasin/constant/g
@@ -0,0 +1,21 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class uniformDimensionedVectorField;
+ location "constant";
+ object g;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 1 -2 0 0 0 0];
+value (0 0 -9.81);
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/iobasin/constant/transportProperties b/tutorials/multiphase/interIsoFoam/iobasin/constant/transportProperties
new file mode 100644
index 0000000000000000000000000000000000000000..c4ebbfe29dd3d8e34d8fb6a8e32cf1a887c4d03c
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/iobasin/constant/transportProperties
@@ -0,0 +1,37 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "constant";
+ object transportProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+phases (water air);
+
+water
+{
+ transportModel Newtonian;
+ nu 1e-06;
+ rho 1000;
+}
+
+air
+{
+ transportModel Newtonian;
+ nu 1.48e-05;
+ rho 1;
+}
+
+sigma 0.07;
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/iobasin/constant/turbulenceProperties b/tutorials/multiphase/interIsoFoam/iobasin/constant/turbulenceProperties
new file mode 100644
index 0000000000000000000000000000000000000000..0077473d45b3cd3f56918e169988a7137ce53d87
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/iobasin/constant/turbulenceProperties
@@ -0,0 +1,20 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "constant";
+ object turbulenceProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType laminar;
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/iobasin/system/blockMeshDict b/tutorials/multiphase/interIsoFoam/iobasin/system/blockMeshDict
new file mode 100644
index 0000000000000000000000000000000000000000..56fcf4bc8618fe48e173a4976ea0c9e00fa75f93
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/iobasin/system/blockMeshDict
@@ -0,0 +1,179 @@
+/*--------------------------------*- C++ -*----------------------------------*/
+
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+scale 1;
+
+// Basin
+x0 0;
+x1 1;
+y0 0;
+y1 1;
+z0 0;
+z1 1;
+
+// Inlet
+x2 -0.3;
+x3 0;
+y2 0.35;
+y3 0.65;
+z2 0.6;
+z3 0.9;
+
+// Outlet
+x4 1;
+x5 1.3;
+y4 0.35;
+y5 0.65;
+z4 0.1;
+z5 0.4;
+
+
+vertices
+(
+ // Basin
+ ($x0 $y0 $z0)
+ ($x1 $y0 $z0)
+ ($x1 $y1 $z0)
+ ($x0 $y1 $z0)
+ ($x0 $y0 $z1)
+ ($x1 $y0 $z1)
+ ($x1 $y1 $z1)
+ ($x0 $y1 $z1)
+
+ // Inlet
+ ($x2 $y2 $z2)
+ ($x3 $y2 $z2)
+ ($x3 $y3 $z2)
+ ($x2 $y3 $z2)
+ ($x2 $y2 $z3)
+ ($x3 $y2 $z3)
+ ($x3 $y3 $z3)
+ ($x2 $y3 $z3)
+
+ // Outlet
+ ($x4 $y4 $z4)
+ ($x5 $y4 $z4)
+ ($x5 $y5 $z4)
+ ($x4 $y5 $z4)
+ ($x4 $y4 $z5)
+ ($x5 $y4 $z5)
+ ($x5 $y5 $z5)
+ ($x4 $y5 $z5)
+);
+
+blocks
+(
+ hex (0 1 2 3 4 5 6 7) (40 40 40) simpleGrading (1 1 1)
+ hex (8 9 10 11 12 13 14 15) (12 12 12) simpleGrading (1 1 1)
+ hex (16 17 18 19 20 21 22 23) (12 12 12) simpleGrading (1 1 1)
+);
+
+boundary
+(
+ inlet
+ {
+ type patch;
+ faces
+ (
+ (8 12 15 11)
+ );
+ }
+
+ outlet
+ {
+ type patch;
+ faces
+ (
+ (17 18 22 21)
+ );
+ }
+
+ walls
+ {
+ type patch;
+ faces
+ (
+ // Basin
+ (0 3 2 1)
+ (0 1 5 4)
+ (2 3 7 6)
+
+ // Inlet
+ (8 11 10 9)
+ (8 9 13 12)
+ (10 11 15 14)
+ (12 13 14 15)
+
+ // Outlet
+ (16 19 18 17)
+ (16 17 21 20)
+ (18 19 23 22)
+ (20 21 22 23)
+ );
+ }
+
+ atmosphere
+ {
+ type patch;
+ faces
+ (
+ (4 5 6 7)
+ );
+ }
+
+ inletRightPatch
+ {
+ type patch;
+ faces
+ (
+ (9 10 14 13)
+ );
+ }
+
+ basinLeftPatch
+ {
+ type patch;
+ faces
+ (
+ (0 4 7 3)
+ );
+ }
+
+ outletLeftPatch
+ {
+ type patch;
+ faces
+ (
+ (16 20 23 19)
+ );
+ }
+
+ basinRightPatch
+ {
+ type patch;
+ faces
+ (
+ (1 2 6 5)
+ );
+ }
+);
+
+edges
+(
+);
+
+mergePatchPairs
+(
+ (inletRightPatch basinLeftPatch)
+ (outletLeftPatch basinRightPatch)
+);
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/iobasin/system/controlDict b/tutorials/multiphase/interIsoFoam/iobasin/system/controlDict
new file mode 100644
index 0000000000000000000000000000000000000000..4b7fd592554c4d40dfd47dcca90338f3b6c23ca2
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/iobasin/system/controlDict
@@ -0,0 +1,100 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2;
+ format ascii;
+ class dictionary;
+ location "system";
+ object controlDict;
+}
+
+application interIsoFoam;
+
+startFrom latestTime;
+
+startTime 0;
+
+stopAt endTime;
+
+endTime 3;
+
+deltaT 0.005;
+//deltaT 0.001;
+
+writeControl adjustableRunTime;
+
+writeInterval 0.01;
+
+purgeWrite 0;
+
+writeFormat binary;
+
+writePrecision 8;
+
+writeCompression off;
+
+timeFormat general;
+
+timePrecision 6;
+
+runTimeModifiable yes;
+
+adjustTimeStep yes;
+
+maxCo 0.8;
+
+maxAlphaCo 0.8;
+
+maxDeltaT 1;
+
+
+functions
+{
+ inletFlux
+ {
+ type surfaceFieldValue;
+ libs ( "libfieldFunctionObjects.so" );
+ writeControl timeStep;
+ log true;
+ writeFields false;
+ regionType patch;
+ name inlet;
+ operation sum;
+ fields ( rhoPhi );
+ }
+
+ outletFlux
+ {
+ type surfaceFieldValue;
+ libs ( "libfieldFunctionObjects.so" );
+ writeControl timeStep;
+ log true;
+ writeFields false;
+ regionType patch;
+ name outlet;
+ operation sum;
+ fields ( rhoPhi );
+ }
+
+ atmosphereFlux
+ {
+ type surfaceFieldValue;
+ libs ( "libfieldFunctionObjects.so" );
+ writeControl timeStep;
+ log true;
+ writeFields false;
+ regionType patch;
+ name atmosphere;
+ operation sum;
+ fields ( rhoPhi );
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/iobasin/system/createPatchDict b/tutorials/multiphase/interIsoFoam/iobasin/system/createPatchDict
new file mode 100644
index 0000000000000000000000000000000000000000..f039ada7f52b3d71b9b46145fcf68d82b6bd10f1
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/iobasin/system/createPatchDict
@@ -0,0 +1,84 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object createPatchDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+pointSync false;
+
+// Patches to create.
+patches
+(
+ {
+ // Name of new patch
+ name walls;
+
+ // Dictionary to construct new patch from
+ patchInfo
+ {
+ type patch;
+ }
+
+ // How to construct: either from 'patches' or 'set'
+ constructFrom patches;
+
+ // If constructFrom = patches : names of patches. Wildcards allowed.
+ patches (walls basinLeftPatch basinRightPatch);
+
+ // If constructFrom = set : name of faceSet
+ set f0;
+ }
+/*
+ {
+ // Name of new patch
+ name walls;
+
+ // Dictionary to construct new patch from
+ patchInfo
+ {
+ type wall;
+ }
+
+ // How to construct: either from 'patches' or 'set'
+ constructFrom patches;
+
+ // If constructFrom = patches : names of patches. Wildcards allowed.
+ patches (originalPatch);
+
+ // If constructFrom = set : name of faceSet
+ set f0;
+ }
+
+ {
+ // Name of new patch
+ name frontAndBack;
+
+ // Dictionary to construct new patch from
+ patchInfo
+ {
+ type empty;
+ }
+
+ // How to construct: either from 'patches' or 'set'
+ constructFrom patches;
+
+ // If constructFrom = patches : names of patches. Wildcards allowed.
+ patches (sides);
+
+ // If constructFrom = set : name of faceSet
+ set f0;
+ }
+*/
+);
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/iobasin/system/decomposeParDict b/tutorials/multiphase/interIsoFoam/iobasin/system/decomposeParDict
new file mode 100644
index 0000000000000000000000000000000000000000..56c7dca5aa46fcac79f99c4044b2e6378be7c495
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/iobasin/system/decomposeParDict
@@ -0,0 +1,28 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ note "mesh decomposition control dictionary";
+ object decomposeParDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains 8;
+
+method simple;
+
+simpleCoeffs
+{
+ n (2 2 2);
+ delta 0.001;
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/iobasin/system/fvSchemes b/tutorials/multiphase/interIsoFoam/iobasin/system/fvSchemes
new file mode 100644
index 0000000000000000000000000000000000000000..e503f16cd74f4dccdab61f7bc5188ea7a3020d5a
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/iobasin/system/fvSchemes
@@ -0,0 +1,64 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+ default Euler;
+}
+
+gradSchemes
+{
+ default Gauss linear;
+}
+
+divSchemes
+{
+ default none;
+ div(rhoPhi,U) Gauss limitedLinearV 1;
+ div(phi,alpha) Gauss vanLeer;
+ div(phirb,alpha) Gauss linear;
+
+ "div\(phi,(k|omega)\)" Gauss upwind;
+ div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
+
+ div(phi,s) Gauss vanLeer;
+ div(phirb,s) Gauss linear;
+}
+
+laplacianSchemes
+{
+ default Gauss linear corrected;
+}
+
+interpolationSchemes
+{
+ default linear;
+}
+
+snGradSchemes
+{
+ default corrected;
+}
+
+/*
+wallDist
+{
+ method meshWave;
+}
+*/
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/iobasin/system/fvSolution b/tutorials/multiphase/interIsoFoam/iobasin/system/fvSolution
new file mode 100644
index 0000000000000000000000000000000000000000..2280dbc593e1ab16aefbf7a4798252e319d92164
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/iobasin/system/fvSolution
@@ -0,0 +1,89 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+ "alpha.water.*"
+ {
+ nAlphaSubCycles 1;
+ cAlpha 1;
+ }
+
+ "pcorr.*"
+ {
+ solver PCG;
+ preconditioner
+ {
+ preconditioner GAMG;
+ tolerance 1e-5;
+ relTol 0;
+ smoother GaussSeidel;
+ }
+ tolerance 1e-5;
+ relTol 0;
+ maxIter 50;
+ }
+
+ p_rgh
+ {
+ solver GAMG;
+ tolerance 5e-9;
+ relTol 0.01;
+
+ smoother GaussSeidel;
+
+
+
+ maxIter 50;
+ };
+
+ p_rghFinal
+ {
+ $p_rgh;
+ tolerance 5e-9;
+ relTol 0;
+ }
+
+ "(U|k|omega|s).*"
+ {
+ solver smoothSolver;
+ smoother symGaussSeidel;
+ nSweeps 1;
+ tolerance 1e-6;
+ relTol 0.1;
+ };
+}
+
+PIMPLE
+{
+ momentumPredictor no;
+ nCorrectors 2;
+ nNonOrthogonalCorrectors 0;
+ pRefCell 0;
+ pRefValue 0;
+}
+
+relaxationFactors
+{
+ equations
+ {
+ ".*" 1;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/iobasin/system/setFieldsDict b/tutorials/multiphase/interIsoFoam/iobasin/system/setFieldsDict
new file mode 100644
index 0000000000000000000000000000000000000000..4424ae1279a1a21d352e1fed6d91600f3444bbe8
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/iobasin/system/setFieldsDict
@@ -0,0 +1,46 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object setFieldsDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+defaultFieldValues
+(
+ volScalarFieldValue alpha.water 0
+);
+
+regions
+(
+ boxToCell
+ {
+ box (-1e10 -1e10 -1e10) (1e10 1e10 0.45);
+ fieldValues
+ (
+ volScalarFieldValue alpha.water 1
+ );
+ }
+
+ boxToCell
+ {
+ box (-1e10 -1e10 -1e10) (-.2 1e10 1e10);
+ fieldValues
+ (
+ volScalarFieldValue alpha.water 1
+ );
+ }
+
+);
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/0.orig/U b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/0.orig/U
new file mode 100644
index 0000000000000000000000000000000000000000..020c0cd55c52841759705c679e54d556b638f505
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/0.orig/U
@@ -0,0 +1,54 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volVectorField;
+ location "0";
+ object U;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 1 -1 0 0 0 0];
+
+internalField uniform (0 0 0);
+
+boundaryField
+{
+ inlet
+ {
+ type waveVelocity;
+ value uniform (0 0 0);
+ }
+
+ outlet
+ {
+ type waveVelocity;
+ value uniform (0 0 0);
+ }
+
+ sides
+ {
+ type empty;
+ }
+
+ ground
+ {
+ type fixedValue;
+ value uniform (0 0 0);
+ }
+
+ top
+ {
+ type pressureInletOutletVelocity;
+ value uniform (0 0 0);
+ }
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/0.orig/alpha.water b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/0.orig/alpha.water
new file mode 100644
index 0000000000000000000000000000000000000000..436879eb36706174517ccdcb3849cb6b506d41ba
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/0.orig/alpha.water
@@ -0,0 +1,52 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ object alpha.water;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 0 0 0 0 0 0];
+
+internalField uniform 0;
+
+boundaryField
+{
+ inlet
+ {
+ type waveAlpha;
+ value uniform 0;
+ }
+
+ outlet
+ {
+ type zeroGradient;
+ }
+
+ ground
+ {
+ type zeroGradient;
+ }
+
+ sides
+ {
+ type empty;
+ }
+
+ top
+ {
+ type inletOutlet;
+ inletValue uniform 0;
+ value uniform 0;
+ }
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/0.orig/p_rgh b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/0.orig/p_rgh
new file mode 100644
index 0000000000000000000000000000000000000000..5fe1bb4ade9ede8985c60b0ac325165805d6b884
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/0.orig/p_rgh
@@ -0,0 +1,54 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ object p_rgh;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [1 -1 -2 0 0 0 0];
+
+internalField uniform 0;
+
+boundaryField
+{
+ inlet
+ {
+ type fixedFluxPressure;
+ value uniform 0;
+ }
+
+ outlet
+ {
+ type fixedFluxPressure;
+ value uniform 0;
+ }
+
+ ground
+ {
+ type fixedFluxPressure;
+ value uniform 0;
+ }
+
+ sides
+ {
+ type empty;
+ }
+
+ top
+ {
+ type totalPressure;
+ p0 uniform 0;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/Allclean b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/Allclean
new file mode 100755
index 0000000000000000000000000000000000000000..e2f275d9fd6e6ba843f14fec57e2987e4c8607b3
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/Allclean
@@ -0,0 +1,7 @@
+#!/bin/sh
+cd ${0%/*} || exit 1 # Run from this directory
+. $WM_PROJECT_DIR/bin/tools/CleanFunctions # Tutorial clean functions
+
+cleanCase0
+
+#------------------------------------------------------------------------------
diff --git a/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/Allrun b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/Allrun
new file mode 100755
index 0000000000000000000000000000000000000000..28bf991e627511713c3b915ac0d9998f068ce030
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/Allrun
@@ -0,0 +1,15 @@
+#!/bin/sh
+cd ${0%/*} || exit 1 # Run from this directory
+. $WM_PROJECT_DIR/bin/tools/RunFunctions # Tutorial run functions
+
+restore0Dir
+
+runApplication blockMesh
+
+runApplication decomposePar
+
+runParallel setFields
+
+runParallel $(getApplication)
+
+#------------------------------------------------------------------------------
diff --git a/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/constant/g b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/constant/g
new file mode 100644
index 0000000000000000000000000000000000000000..492b5693e947caf937121bd5e6977ef9dcf59896
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/constant/g
@@ -0,0 +1,22 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class uniformDimensionedVectorField;
+ location "constant";
+ object g;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 1 -2 0 0 0 0];
+value ( 0 0 -9.81 );
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/constant/transportProperties b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/constant/transportProperties
new file mode 100644
index 0000000000000000000000000000000000000000..70f3aebb062ac5bca95ae0908d0ec48ca1de4f8c
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/constant/transportProperties
@@ -0,0 +1,37 @@
+/*---------------------------------------------------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "constant";
+ object transportProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+phases (water air);
+
+water
+{
+ transportModel Newtonian;
+ nu 1e-06;
+ rho 1000;
+}
+
+air
+{
+ transportModel Newtonian;
+ nu 1.48e-05;
+ rho 1;
+}
+
+sigma 0.07;
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/constant/turbulenceProperties b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/constant/turbulenceProperties
new file mode 100644
index 0000000000000000000000000000000000000000..feea4803ea50860c13e81ee1b30d0af0aebcf956
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/constant/turbulenceProperties
@@ -0,0 +1,20 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "constant";
+ object turbulenceProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType laminar;
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/constant/waveProperties b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/constant/waveProperties
new file mode 100644
index 0000000000000000000000000000000000000000..b18ad6d4d2ab6e1e719997a45db91b1271a5289a
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/constant/waveProperties
@@ -0,0 +1,80 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "constant";
+ object waveProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+inlet
+{
+ alpha alpha.water;
+
+ waveModel streamFunction;
+
+ nPaddle 1;
+
+ waveHeight 0.1517;
+
+ waveAngle 0.0;
+
+ rampTime 3.017;//6.034;
+
+ activeAbsorption yes;
+
+ wavePeriod 3.017;
+
+ uMean 2.0825;
+
+ waveLength 6.2832;
+
+ Bjs
+ (
+ 8.6669014e-002
+ 2.4849799e-002
+ 7.7446850e-003
+ 2.3355420e-003
+ 6.4497731e-004
+ 1.5205114e-004
+ 2.5433769e-005
+ -2.2045436e-007
+ -2.8711504e-006
+ -1.2287334e-006
+ );
+
+ Ejs
+ (
+ 5.6009609e-002
+ 3.1638171e-002
+ 1.5375952e-002
+ 7.1743178e-003
+ 3.3737077e-003
+ 1.6324880e-003
+ 8.2331980e-004
+ 4.4403497e-004
+ 2.7580059e-004
+ 2.2810557e-004
+ );
+
+}
+
+outlet
+{
+ alpha alpha.water;
+
+ waveModel shallowWaterAbsorption;
+
+ nPaddle 1;
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/system/blockMeshDict b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/system/blockMeshDict
new file mode 100644
index 0000000000000000000000000000000000000000..7e2390b70576a7b4af0b710acc71f461e1e95bc6
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/system/blockMeshDict
@@ -0,0 +1,91 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+scale 1;
+
+vertices
+(
+ ( 0.0 0.0 0.0)
+ ( 40.0 0.0 0.0)
+ ( 40.0 0.01 0.0)
+ ( 0.0 0.01 0.0)
+ ( 0.0 0.0 0.8)
+ ( 40.0 0.0 0.8)
+ ( 40.0 0.01 0.8)
+ ( 0.0 0.01 0.8)
+);
+
+blocks
+(
+ hex (0 1 2 3 4 5 6 7) (2000 1 80) simpleGrading (1 1 1)
+);
+
+edges
+(
+);
+
+boundary
+(
+ inlet
+ {
+ type patch;
+ faces
+ (
+ (0 4 7 3)
+ );
+ }
+ outlet
+ {
+ type patch;
+ faces
+ (
+ (1 5 6 2)
+ );
+ }
+ ground
+ {
+ type wall;
+ faces
+ (
+ (0 1 2 3)
+ );
+ }
+ top
+ {
+ type patch;
+ faces
+ (
+ (4 5 6 7)
+ );
+ }
+ sides
+ {
+ type empty;
+ faces
+ (
+ (0 1 5 4)
+ (3 2 6 7)
+ );
+ }
+);
+
+mergePatchPairs
+(
+);
+
+// ************************************************************************* //
+
+
diff --git a/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/system/controlDict b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/system/controlDict
new file mode 100644
index 0000000000000000000000000000000000000000..c0cf911c720335e0f12c5a4336dfc552897c229a
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/system/controlDict
@@ -0,0 +1,162 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application interIsoFoam;
+
+startFrom latestTime;
+
+startTime 0;
+
+stopAt endTime;
+
+endTime 30.0;
+
+deltaT 0.001;
+
+writeControl adjustableRunTime;
+
+writeInterval 0.15085;
+
+purgeWrite 0;
+
+writeFormat ascii;
+
+writePrecision 6;
+
+writeCompression off;
+
+timeFormat general;
+
+timePrecision 6;
+
+runTimeModifiable yes;
+
+adjustTimeStep yes;
+
+maxCo 0.5;
+maxAlphaCo 0.5;
+
+maxDeltaT 0.5;
+
+
+functions
+{
+ line
+ {
+ type sets;
+ libs ("libsampling.so");
+ enabled true;
+ writeControl writeTime;
+ writeInterval 1;
+
+ interpolationScheme cellPoint;
+ setFormat raw;
+ sets
+ (
+ line1
+ {
+ type uniform;
+ axis distance;
+ start ( 1.0 0.005 0.0 );
+ end ( 1.0 0.005 1.0 );
+ nPoints 1001;
+ }
+ line2
+ {
+ type uniform;
+ axis distance;
+ start ( 2.0 0.005 0.0 );
+ end ( 2.0 0.005 1.0 );
+ nPoints 1001;
+ }
+ line3
+ {
+ type uniform;
+ axis distance;
+ start ( 3.0 0.005 0.0 );
+ end ( 3.0 0.005 1.0 );
+ nPoints 1001;
+ }
+ line4
+ {
+ type uniform;
+ axis distance;
+ start ( 5.0 0.005 0.0 );
+ end ( 5.0 0.005 1.0 );
+ nPoints 1001;
+ }
+ line5
+ {
+ type uniform;
+ axis distance;
+ start ( 7.5 0.005 0.0 );
+ end ( 7.5 0.005 1.0 );
+ nPoints 1001;
+ }
+
+ line6
+ {
+ type uniform;
+ axis distance;
+ start ( 10.0 0.005 0.0 );
+ end ( 10.0 0.005 1.0 );
+ nPoints 1001;
+ }
+ line7
+ {
+ type uniform;
+ axis distance;
+ start ( 12.0 0.005 0.0 );
+ end ( 12.0 0.005 1.0 );
+ nPoints 1001;
+ }
+ line8
+ {
+ type uniform;
+ axis distance;
+ start ( 15.0 0.005 0.0 );
+ end ( 15.0 0.005 1.0 );
+ nPoints 1001;
+ }
+ line9
+ {
+ type uniform;
+ axis distance;
+ start ( 20.0 0.005 0.0 );
+ end ( 20.0 0.005 1.0 );
+ nPoints 1001;
+ }
+ line10
+ {
+ type uniform;
+ axis distance;
+ start ( 28.0 0.005 0.0 );
+ end ( 28.0 0.005 1.0 );
+ nPoints 1001;
+ }
+ );
+
+ fixedLocations false;
+ fields
+ (
+ U alpha.water
+ );
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/system/decomposeParDict b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/system/decomposeParDict
new file mode 100644
index 0000000000000000000000000000000000000000..d17ee03e3d140ed6365240ae578a9571b03f25b9
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/system/decomposeParDict
@@ -0,0 +1,29 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object decomposeParDict;
+}
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains 2;
+
+method hierarchical;
+
+hierarchicalCoeffs
+{
+ n (2 1 1);
+ delta 0.001;
+ order xyz;
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/system/fvSchemes b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/system/fvSchemes
new file mode 100644
index 0000000000000000000000000000000000000000..1962d3a4a4c428c507a2c1abc4829eda87a7ab3e
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/system/fvSchemes
@@ -0,0 +1,54 @@
+
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+ default Euler;
+}
+
+gradSchemes
+{
+ default Gauss linear;
+}
+
+divSchemes
+{
+ div(rhoPhi,U) Gauss linearUpwind grad(U);
+ div(phi,alpha) Gauss vanLeer;
+ div(phirb,alpha) Gauss linear;
+ div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
+}
+
+laplacianSchemes
+{
+ default Gauss linear orthogonal;
+}
+
+interpolationSchemes
+{
+ default linear;
+}
+
+snGradSchemes
+{
+ default orthogonal;
+}
+
+
+// ************************************************************************* //
+
diff --git a/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/system/fvSolution b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/system/fvSolution
new file mode 100644
index 0000000000000000000000000000000000000000..46b73f7e0c00bae63f435b4bebd71f8c40c86767
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/system/fvSolution
@@ -0,0 +1,89 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+ "alpha.water.*"
+ {
+ isoFaceTol 1e-10;
+ surfCellTol 1e-2;
+ nAlphaBounds 3;
+ snapTol 1e-12;
+ clip true;
+
+ nAlphaCorr 1;
+ nAlphaSubCycles 1;
+ cAlpha 1;
+
+ MULESCorr yes;
+ nLimiterIter 5;
+
+ solver smoothSolver;
+ smoother symGaussSeidel;
+ tolerance 1e-8;
+ relTol 0;
+ }
+
+ "pcorr.*"
+ {
+ solver PCG;
+ preconditioner DIC;
+ tolerance 1e-6;
+ relTol 0;
+ }
+
+ p_rgh
+ {
+ solver PCG;
+ preconditioner DIC;
+ tolerance 1e-08;
+ relTol 0.05;
+ }
+
+ p_rghFinal
+ {
+ $p_rgh;
+ relTol 0;
+ }
+
+ U
+ {
+ solver smoothSolver;
+ smoother symGaussSeidel;
+ tolerance 1e-06;
+ relTol 0;
+ }
+}
+
+PIMPLE
+{
+ momentumPredictor no;
+ nOuterCorrectors 1;
+ nCorrectors 3;
+ nNonOrthogonalCorrectors 0;
+}
+
+relaxationFactors
+{
+ equations
+ {
+ ".*" 1;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/system/setFieldsDict b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/system/setFieldsDict
new file mode 100644
index 0000000000000000000000000000000000000000..bbf3c8d43fc1769aa3461f2c9dfb6f2c26d43523
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/waveExampleStreamFunction/system/setFieldsDict
@@ -0,0 +1,36 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object setFieldsDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+defaultFieldValues
+(
+ volScalarFieldValue alpha.water 0
+);
+
+regions
+(
+ boxToCell
+ {
+ box (0 0 0) (40.0 1.0 0.4046);
+ fieldValues
+ (
+ volScalarFieldValue alpha.water 1
+ );
+ }
+);
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/weirOverflow/0.orig/U b/tutorials/multiphase/interIsoFoam/weirOverflow/0.orig/U
new file mode 100644
index 0000000000000000000000000000000000000000..615644c61b1ad1f0eadeba1bceb00e72827b151a
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/weirOverflow/0.orig/U
@@ -0,0 +1,55 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volVectorField;
+ object U;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#include "include/initialConditions"
+
+dimensions [0 1 -1 0 0 0 0];
+
+internalField uniform (0 0 0);
+
+boundaryField
+{
+ inlet
+ {
+ type variableHeightFlowRateInletVelocity;
+ flowRate $inletFlowRate;
+ alpha alpha.water;
+ value uniform (0 0 0);
+ }
+
+ outlet
+ {
+ type zeroGradient;
+ }
+
+ lowerWall
+ {
+ type noSlip;
+ }
+
+ atmosphere
+ {
+ type pressureInletOutletVelocity;
+ value uniform (0 0 0);
+ }
+
+ defaultFaces
+ {
+ type empty;
+ }
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/weirOverflow/0.orig/alpha.water.orig b/tutorials/multiphase/interIsoFoam/weirOverflow/0.orig/alpha.water.orig
new file mode 100644
index 0000000000000000000000000000000000000000..7562548261e83ddce3406ae902c4fca9dc6b1a5f
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/weirOverflow/0.orig/alpha.water.orig
@@ -0,0 +1,56 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ object alpha.water;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#include "include/initialConditions"
+
+dimensions [0 0 0 0 0 0 0];
+
+internalField uniform 0;
+
+boundaryField
+{
+ inlet
+ {
+ type variableHeightFlowRate;
+ lowerBound 0;
+ upperBound 1;
+ value uniform 0;
+ }
+
+ outlet
+ {
+ type zeroGradient;
+ }
+
+ lowerWall
+ {
+ type zeroGradient;
+ }
+
+ atmosphere
+ {
+ type inletOutlet;
+ inletValue uniform 0;
+ value uniform 0;
+ }
+
+ defaultFaces
+ {
+ type empty;
+ }
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/weirOverflow/0.orig/epsilon b/tutorials/multiphase/interIsoFoam/weirOverflow/0.orig/epsilon
new file mode 100644
index 0000000000000000000000000000000000000000..e4501081b331459a602d3651758f86a931840ad8
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/weirOverflow/0.orig/epsilon
@@ -0,0 +1,59 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object epsilon;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#include "include/initialConditions"
+
+dimensions [0 2 -3 0 0 0 0];
+
+internalField uniform $turbulentEpsilon;
+
+boundaryField
+{
+ inlet
+ {
+ type fixedValue;
+ value $internalField;
+ }
+
+ outlet
+ {
+ type inletOutlet;
+ inletValue $internalField;
+ value $internalField;
+ }
+
+ lowerWall
+ {
+ type epsilonWallFunction;
+ value $internalField;
+ }
+
+ atmosphere
+ {
+ type inletOutlet;
+ inletValue $internalField;
+ value $internalField;
+ }
+
+ defaultFaces
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/weirOverflow/0.orig/include/initialConditions b/tutorials/multiphase/interIsoFoam/weirOverflow/0.orig/include/initialConditions
new file mode 100644
index 0000000000000000000000000000000000000000..2331b854d28b7f57489fe2be1830c3c47874e8d3
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/weirOverflow/0.orig/include/initialConditions
@@ -0,0 +1,14 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+
+inletFlowRate 75;
+pressure 0;
+turbulentKE 4.14e-03;
+turbulentEpsilon 4.39e-05;
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/weirOverflow/0.orig/k b/tutorials/multiphase/interIsoFoam/weirOverflow/0.orig/k
new file mode 100644
index 0000000000000000000000000000000000000000..1b0b46e5dcaef99f1081fbf546e61188d378e695
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/weirOverflow/0.orig/k
@@ -0,0 +1,59 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object k;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#include "include/initialConditions"
+
+dimensions [0 2 -2 0 0 0 0];
+
+internalField uniform $turbulentKE;
+
+boundaryField
+{
+ inlet
+ {
+ type fixedValue;
+ value $internalField;
+ }
+
+ outlet
+ {
+ type inletOutlet;
+ inletValue $internalField;
+ value $internalField;
+ }
+
+ lowerWall
+ {
+ type kqRWallFunction;
+ value $internalField;
+ }
+
+ atmosphere
+ {
+ type inletOutlet;
+ inletValue $internalField;
+ value $internalField;
+ }
+
+ defaultFaces
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/weirOverflow/0.orig/nut b/tutorials/multiphase/interIsoFoam/weirOverflow/0.orig/nut
new file mode 100644
index 0000000000000000000000000000000000000000..7af6950d8bb11a89b8e1d78517e84a0d7a59c2db
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/weirOverflow/0.orig/nut
@@ -0,0 +1,52 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object nut;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 2 -1 0 0 0 0];
+
+internalField uniform 0;
+
+boundaryField
+{
+ inlet
+ {
+ type calculated;
+ value uniform 0;
+ }
+ outlet
+ {
+ type calculated;
+ value uniform 0;
+ }
+ lowerWall
+ {
+ type nutkWallFunction;
+ value uniform 0;
+ }
+ atmosphere
+ {
+ type calculated;
+ value uniform 0;
+ }
+
+ defaultFaces
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/weirOverflow/0.orig/p_rgh b/tutorials/multiphase/interIsoFoam/weirOverflow/0.orig/p_rgh
new file mode 100644
index 0000000000000000000000000000000000000000..e692f6e849060bc15026c5b807b25dfe3d26fdbc
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/weirOverflow/0.orig/p_rgh
@@ -0,0 +1,52 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ object p_rgh;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#include "include/initialConditions"
+
+dimensions [1 -1 -2 0 0 0 0];
+
+internalField uniform $pressure;
+
+boundaryField
+{
+ inlet
+ {
+ type zeroGradient;
+ }
+
+ outlet
+ {
+ type zeroGradient;
+ }
+
+ lowerWall
+ {
+ type fixedFluxPressure;
+ }
+
+ atmosphere
+ {
+ type totalPressure;
+ p0 uniform 0;
+ }
+
+ defaultFaces
+ {
+ type empty;
+ }
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/weirOverflow/Allclean b/tutorials/multiphase/interIsoFoam/weirOverflow/Allclean
new file mode 100755
index 0000000000000000000000000000000000000000..e2f275d9fd6e6ba843f14fec57e2987e4c8607b3
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/weirOverflow/Allclean
@@ -0,0 +1,7 @@
+#!/bin/sh
+cd ${0%/*} || exit 1 # Run from this directory
+. $WM_PROJECT_DIR/bin/tools/CleanFunctions # Tutorial clean functions
+
+cleanCase0
+
+#------------------------------------------------------------------------------
diff --git a/tutorials/multiphase/interIsoFoam/weirOverflow/Allrun b/tutorials/multiphase/interIsoFoam/weirOverflow/Allrun
new file mode 100755
index 0000000000000000000000000000000000000000..c7107259267d9ec3d57107003fcfe6a9e1483ad5
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/weirOverflow/Allrun
@@ -0,0 +1,13 @@
+#!/bin/sh
+cd ${0%/*} || exit 1 # Run from this directory
+. $WM_PROJECT_DIR/bin/tools/RunFunctions # Tutorial run functions
+
+restore0Dir
+
+runApplication blockMesh
+\cp 0/alpha.water.orig 0/alpha.water
+
+runApplication setFields
+runApplication $(getApplication)
+
+#------------------------------------------------------------------------------
diff --git a/tutorials/multiphase/interIsoFoam/weirOverflow/constant/g b/tutorials/multiphase/interIsoFoam/weirOverflow/constant/g
new file mode 100644
index 0000000000000000000000000000000000000000..037697dd981e91821b2f945f442f842357790ef0
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/weirOverflow/constant/g
@@ -0,0 +1,22 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class uniformDimensionedVectorField;
+ location "constant";
+ object g;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 1 -2 0 0 0 0];
+value (0 -9.81 0);
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/weirOverflow/constant/transportProperties b/tutorials/multiphase/interIsoFoam/weirOverflow/constant/transportProperties
new file mode 100644
index 0000000000000000000000000000000000000000..c4ebbfe29dd3d8e34d8fb6a8e32cf1a887c4d03c
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/weirOverflow/constant/transportProperties
@@ -0,0 +1,37 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "constant";
+ object transportProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+phases (water air);
+
+water
+{
+ transportModel Newtonian;
+ nu 1e-06;
+ rho 1000;
+}
+
+air
+{
+ transportModel Newtonian;
+ nu 1.48e-05;
+ rho 1;
+}
+
+sigma 0.07;
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/weirOverflow/constant/turbulenceProperties b/tutorials/multiphase/interIsoFoam/weirOverflow/constant/turbulenceProperties
new file mode 100644
index 0000000000000000000000000000000000000000..0e5f55ae375d8a8f5549782d89481e69caeb1861
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/weirOverflow/constant/turbulenceProperties
@@ -0,0 +1,30 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "constant";
+ object turbulenceProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType RAS;
+
+RAS
+{
+ RASModel kEpsilon;
+
+ turbulence on;
+
+ printCoeffs on;
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/weirOverflow/system/blockMeshDict b/tutorials/multiphase/interIsoFoam/weirOverflow/system/blockMeshDict
new file mode 100644
index 0000000000000000000000000000000000000000..c8309631490290d3683ac35899511f556db603f2
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/weirOverflow/system/blockMeshDict
@@ -0,0 +1,93 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+scale 1;
+
+vertices
+(
+ (-18 0 -0.5)
+ ( 0 0 -0.5)
+ ( 30 0 -0.5)
+ ( 90 0 -0.5)
+ (-18 30 -0.5)
+ ( 0 30 -0.5)
+ ( 15 30 -0.5)
+ ( 90 30 -0.5)
+ (-18 54 -0.5)
+ ( 0 54 -0.5)
+ ( 15 54 -0.5)
+ ( 90 54 -0.5)
+
+ (-18 0 0.5)
+ ( 0 0 0.5)
+ ( 30 0 0.5)
+ ( 90 0 0.5)
+ (-18 30 0.5)
+ ( 0 30 0.5)
+ ( 15 30 0.5)
+ ( 90 30 0.5)
+ (-18 54 0.5)
+ ( 0 54 0.5)
+ ( 15 54 0.5)
+ ( 90 54 0.5)
+);
+
+blocks
+(
+ hex (0 1 5 4 12 13 17 16) (20 20 1) simpleGrading (1 0.5 1)
+ hex (2 3 7 6 14 15 19 18) (60 40 1) simpleGrading (1 2 1)
+ hex (4 5 9 8 16 17 21 20) (20 24 1) simpleGrading (1 1 1)
+ hex (5 6 10 9 17 18 22 21) (15 24 1) simpleGrading (1 1 1)
+ hex (6 7 11 10 18 19 23 22) (60 24 1) simpleGrading (1 1 1)
+);
+
+edges
+(
+);
+
+patches
+(
+ patch inlet
+ (
+ (0 12 16 4)
+ (4 16 20 8)
+ )
+ patch outlet
+ (
+ (7 19 15 3)
+ (11 23 19 7)
+ )
+ wall lowerWall
+ (
+ (0 1 13 12)
+ (1 5 17 13)
+ (5 6 18 17)
+ (2 14 18 6)
+ (2 3 15 14)
+ )
+ patch atmosphere
+ (
+ (8 20 21 9)
+ (9 21 22 10)
+ (10 22 23 11)
+ )
+);
+
+mergePatchPairs
+(
+);
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/weirOverflow/system/controlDict b/tutorials/multiphase/interIsoFoam/weirOverflow/system/controlDict
new file mode 100644
index 0000000000000000000000000000000000000000..1b57380eefa56a1b689ead25bfa07e5554573c98
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/weirOverflow/system/controlDict
@@ -0,0 +1,55 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application interIsoFoam;
+
+startFrom latestTime;
+
+startTime 0;
+
+stopAt endTime;
+
+endTime 30;
+
+deltaT 0.001;
+
+writeControl adjustableRunTime;
+
+writeInterval 2;
+
+purgeWrite 0;
+
+writeFormat ascii;
+
+writePrecision 6;
+
+writeCompression off;
+
+timeFormat general;
+
+timePrecision 6;
+
+runTimeModifiable yes;
+
+adjustTimeStep on;
+
+maxCo 0.9;
+maxAlphaCo 0.9;
+
+maxDeltaT 1;
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/weirOverflow/system/fvSchemes b/tutorials/multiphase/interIsoFoam/weirOverflow/system/fvSchemes
new file mode 100644
index 0000000000000000000000000000000000000000..7b9531750a95c9a937f24b03ff552b3ea7740e7f
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/weirOverflow/system/fvSchemes
@@ -0,0 +1,56 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+ default Euler;
+}
+
+gradSchemes
+{
+ default Gauss linear;
+}
+
+divSchemes
+{
+ div(rhoPhi,U) Gauss linear;
+ div(phi,alpha) Gauss vanLeer;
+ div(phirb,alpha) Gauss linear;
+ div(phi,k) Gauss upwind;
+ div(phi,epsilon) Gauss upwind;
+ div(phi,R) Gauss upwind;
+ div(R) Gauss linear;
+ div(phi,nuTilda) Gauss upwind;
+ div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
+}
+
+laplacianSchemes
+{
+ default Gauss linear corrected;
+}
+
+interpolationSchemes
+{
+ default linear;
+}
+
+snGradSchemes
+{
+ default corrected;
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/weirOverflow/system/fvSolution b/tutorials/multiphase/interIsoFoam/weirOverflow/system/fvSolution
new file mode 100644
index 0000000000000000000000000000000000000000..6ff4f3463f969a9a54133f251a2d810896142401
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/weirOverflow/system/fvSolution
@@ -0,0 +1,79 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+ alpha.water
+ {
+
+ isoFaceTol 1e-6;
+ surfCellTol 1e-6;
+ nAlphaBounds 3;
+ snapTol 1e-12;
+ clip true;
+
+ nAlphaSubCycles 1;
+ cAlpha 1; // Note: cAlpha is not used by isoAdvector but must
+ // be specified because interfacePropertes object
+ // reads it during construction.
+ }
+
+ "pcorr.*"
+ {
+ solver PCG;
+ preconditioner DIC;
+ tolerance 1e-10;
+ relTol 0;
+ }
+
+ p_rgh
+ {
+ solver PCG;
+ preconditioner DIC;
+ tolerance 1e-08;
+ relTol 0.05;
+ }
+
+ p_rghFinal
+ {
+ $p_rgh;
+ relTol 0;
+ }
+
+ "(U|k|epsilon)"
+ {
+ solver smoothSolver;
+ smoother symGaussSeidel;
+ tolerance 1e-8;
+ relTol 0.1;
+ }
+
+ "(U|k|epsilon)Final"
+ {
+ $U;
+ relTol 0;
+ }
+}
+
+PIMPLE
+{
+ momentumPredictor no;
+ nCorrectors 3;
+ nNonOrthogonalCorrectors 0;
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interIsoFoam/weirOverflow/system/setFieldsDict b/tutorials/multiphase/interIsoFoam/weirOverflow/system/setFieldsDict
new file mode 100644
index 0000000000000000000000000000000000000000..1020eb07ee169c77f4a6dee85cd1971a3bf854e0
--- /dev/null
+++ b/tutorials/multiphase/interIsoFoam/weirOverflow/system/setFieldsDict
@@ -0,0 +1,35 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v1806 |
+| \\ / A nd | Web: www.OpenFOAM.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object setFieldsDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+defaultFieldValues
+(
+ volScalarFieldValue alpha.water 0
+);
+
+regions
+(
+ boxToCell
+ {
+ box (-100 0 -100) (0 20 100);
+
+ fieldValues
+ (
+ volScalarFieldValue alpha.water 1
+ );
+ }
+);
+
+// ************************************************************************* //