diff --git a/tutorials/multiphase/interFoam/laminar/damBreakPermeable/0.orig/U b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/0.orig/U
new file mode 100644
index 0000000000000000000000000000000000000000..7febd45f3b90602badfaaea3398b5a845a61cd52
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/0.orig/U
@@ -0,0 +1,54 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2012 |
+| \\ / A nd | Website: 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 0 0);
+
+boundaryField
+{
+ leftWall
+ {
+ type noSlip;
+ }
+
+ rightWall
+ {
+ type permeableAlphaPressureInletOutletVelocity;
+ alpha alpha.water;
+ alphaMin 0.01;
+ value uniform (0 0 0);
+ }
+
+ lowerWall
+ {
+ type noSlip;
+ }
+
+ atmosphere
+ {
+ type pressureInletOutletVelocity;
+ value uniform (0 0 0);
+ }
+
+ defaultFaces
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/damBreakPermeable/0.orig/alpha.water b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/0.orig/alpha.water
new file mode 100644
index 0000000000000000000000000000000000000000..721ca601150436bf5071551166f213f396fbff5d
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/0.orig/alpha.water
@@ -0,0 +1,52 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2012 |
+| \\ / A nd | Website: 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
+{
+ leftWall
+ {
+ type zeroGradient;
+ }
+
+ rightWall
+ {
+ type zeroGradient;
+ }
+
+ lowerWall
+ {
+ type zeroGradient;
+ }
+
+ atmosphere
+ {
+ type inletOutlet;
+ inletValue uniform 0;
+ value uniform 0;
+ }
+
+ defaultFaces
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/damBreakPermeable/0.orig/epsilon b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/0.orig/epsilon
new file mode 100644
index 0000000000000000000000000000000000000000..1ba6569c5997bdc3497fcf5bf8a96241006e3b3b
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/0.orig/epsilon
@@ -0,0 +1,55 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2012 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ object epsilon;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 2 -3 0 0 0 0];
+
+internalField uniform 0.1;
+
+boundaryField
+{
+ leftWall
+ {
+ type epsilonWallFunction;
+ value uniform 0.1;
+ }
+
+ rightWall
+ {
+ type epsilonWallFunction;
+ value uniform 0.1;
+ }
+
+ lowerWall
+ {
+ type epsilonWallFunction;
+ value uniform 0.1;
+ }
+
+ atmosphere
+ {
+ type inletOutlet;
+ inletValue uniform 0.1;
+ value uniform 0.1;
+ }
+
+ defaultFaces
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/damBreakPermeable/0.orig/k b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/0.orig/k
new file mode 100644
index 0000000000000000000000000000000000000000..7d0e56de178fa44a2a3848914557b8ae0fcb687d
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/0.orig/k
@@ -0,0 +1,55 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2012 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ object k;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 2 -2 0 0 0 0];
+
+internalField uniform 0.1;
+
+boundaryField
+{
+ leftWall
+ {
+ type kqRWallFunction;
+ value uniform 0.1;
+ }
+
+ rightWall
+ {
+ type kqRWallFunction;
+ value uniform 0.1;
+ }
+
+ lowerWall
+ {
+ type kqRWallFunction;
+ value uniform 0.1;
+ }
+
+ atmosphere
+ {
+ type inletOutlet;
+ inletValue uniform 0.1;
+ value uniform 0.1;
+ }
+
+ defaultFaces
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/damBreakPermeable/0.orig/nut b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/0.orig/nut
new file mode 100644
index 0000000000000000000000000000000000000000..8bd8fdd6a568db58bc27e62ffa611cdb5d3c3701
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/0.orig/nut
@@ -0,0 +1,54 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2012 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ object nut;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 2 -1 0 0 0 0];
+
+internalField uniform 0;
+
+boundaryField
+{
+ leftWall
+ {
+ type nutkWallFunction;
+ value uniform 0;
+ }
+
+ rightWall
+ {
+ type nutkWallFunction;
+ value uniform 0;
+ }
+
+ lowerWall
+ {
+ type nutkWallFunction;
+ value uniform 0;
+ }
+
+ atmosphere
+ {
+ type calculated;
+ value uniform 0;
+ }
+
+ defaultFaces
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/damBreakPermeable/0.orig/p_rgh b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/0.orig/p_rgh
new file mode 100644
index 0000000000000000000000000000000000000000..96a5b6c493d480d57986f75349cbf3289c1ce75d
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/0.orig/p_rgh
@@ -0,0 +1,57 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2012 |
+| \\ / A nd | Website: 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
+{
+ leftWall
+ {
+ type fixedFluxPressure;
+ value uniform 0;
+ }
+
+ rightWall
+ {
+ type prghPermeableAlphaTotalPressure;
+ alpha alpha.water;
+ alphaMin 0.01;
+ p uniform 0;
+ value uniform 0;
+ }
+
+ lowerWall
+ {
+ type fixedFluxPressure;
+ value uniform 0;
+ }
+
+ atmosphere
+ {
+ type totalPressure;
+ p0 uniform 0;
+ }
+
+ defaultFaces
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/damBreakPermeable/Allclean b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/Allclean
new file mode 100755
index 0000000000000000000000000000000000000000..fb1f3847301c377e02e12439ba58cbf303af3ef9
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/Allclean
@@ -0,0 +1,8 @@
+#!/bin/sh
+cd "${0%/*}" || exit # Run from this directory
+. ${WM_PROJECT_DIR:?}/bin/tools/CleanFunctions # Tutorial clean functions
+#------------------------------------------------------------------------------
+
+cleanCase0
+
+#------------------------------------------------------------------------------
diff --git a/tutorials/multiphase/interFoam/laminar/damBreakPermeable/Allrun b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/Allrun
new file mode 100755
index 0000000000000000000000000000000000000000..e26a2e10417309a7f9e5a812f9e3e50ca722fe18
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/Allrun
@@ -0,0 +1,18 @@
+#!/bin/sh
+cd "${0%/*}" || exit # Run from this directory
+. ${WM_PROJECT_DIR:?}/bin/tools/RunFunctions # Tutorial run functions
+#------------------------------------------------------------------------------
+
+restore0Dir
+
+runApplication blockMesh
+
+runApplication setFields
+
+runApplication decomposePar
+
+runParallel $(getApplication)
+
+runParallel redistributePar -reconstruct -overwrite
+
+#------------------------------------------------------------------------------
diff --git a/tutorials/multiphase/interFoam/laminar/damBreakPermeable/constant/g b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/constant/g
new file mode 100644
index 0000000000000000000000000000000000000000..28b07d0b8775454e4fb6f1314f165492290a396a
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/constant/g
@@ -0,0 +1,21 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2012 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class uniformDimensionedVectorField;
+ object g;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 1 -2 0 0 0 0];
+value (0 -9.81 0);
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/damBreakPermeable/constant/transportProperties b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/constant/transportProperties
new file mode 100644
index 0000000000000000000000000000000000000000..15c0d5bd12c02dda59fffc7e9b1d915b8abcbc5a
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/constant/transportProperties
@@ -0,0 +1,36 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2012 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ 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/interFoam/laminar/damBreakPermeable/constant/turbulenceProperties b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/constant/turbulenceProperties
new file mode 100644
index 0000000000000000000000000000000000000000..f113b8d4078c0a15fba49dd6fbb3965f470968e0
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/constant/turbulenceProperties
@@ -0,0 +1,31 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2012 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object turbulenceProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType RAS;
+
+density variable;
+
+RAS
+{
+ RASModel kEpsilon;
+
+ turbulence on;
+
+ printCoeffs on;
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/damBreakPermeable/system/blockMeshDict b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/system/blockMeshDict
new file mode 100644
index 0000000000000000000000000000000000000000..867860524d7db076ba20d4e5a2610eebcfe5f448
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/system/blockMeshDict
@@ -0,0 +1,109 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2012 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+scale 0.146;
+
+vertices
+(
+ (0 0 0)
+ (2 0 0)
+ (2.16438 0 0)
+ (4 0 0)
+ (0 0.32876 0)
+ (2 0.32876 0)
+ (2.16438 0.32876 0)
+ (4 0.32876 0)
+ (0 4 0)
+ (2 4 0)
+ (2.16438 4 0)
+ (4 4 0)
+ (0 0 0.1)
+ (2 0 0.1)
+ (2.16438 0 0.1)
+ (4 0 0.1)
+ (0 0.32876 0.1)
+ (2 0.32876 0.1)
+ (2.16438 0.32876 0.1)
+ (4 0.32876 0.1)
+ (0 4 0.1)
+ (2 4 0.1)
+ (2.16438 4 0.1)
+ (4 4 0.1)
+);
+
+blocks
+(
+ hex (0 1 5 4 12 13 17 16) (23 8 1) simpleGrading (1 1 1)
+ hex (2 3 7 6 14 15 19 18) (19 8 1) simpleGrading (1 1 1)
+ hex (4 5 9 8 16 17 21 20) (23 42 1) simpleGrading (1 1 1)
+ hex (5 6 10 9 17 18 22 21) (4 42 1) simpleGrading (1 1 1)
+ hex (6 7 11 10 18 19 23 22) (19 42 1) simpleGrading (1 1 1)
+);
+
+edges
+(
+);
+
+boundary
+(
+ leftWall
+ {
+ type wall;
+ faces
+ (
+ (0 12 16 4)
+ (4 16 20 8)
+ );
+ }
+ rightWall
+ {
+ type wall;
+ faces
+ (
+ (7 19 15 3)
+ (11 23 19 7)
+ );
+ }
+ lowerWall
+ {
+ type wall;
+ faces
+ (
+ (0 1 13 12)
+ (1 5 17 13)
+ (5 6 18 17)
+ (2 14 18 6)
+ (2 3 15 14)
+ );
+ }
+ atmosphere
+ {
+ type patch;
+ faces
+ (
+ (8 20 21 9)
+ (9 21 22 10)
+ (10 22 23 11)
+ );
+ }
+);
+
+mergePatchPairs
+(
+);
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/damBreakPermeable/system/controlDict b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/system/controlDict
new file mode 100644
index 0000000000000000000000000000000000000000..472dac9be27176cf085a8e04945ac5b4be709dcb
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/system/controlDict
@@ -0,0 +1,56 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2012 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application interFoam;
+
+startFrom startTime;
+
+startTime 0;
+
+stopAt endTime;
+
+endTime 1;
+
+deltaT 0.001;
+
+writeControl adjustable;
+
+writeInterval 0.05;
+
+purgeWrite 0;
+
+writeFormat ascii;
+
+writePrecision 6;
+
+writeCompression off;
+
+timeFormat general;
+
+timePrecision 6;
+
+runTimeModifiable yes;
+
+adjustTimeStep on;
+
+maxCo 1;
+
+maxAlphaCo 1;
+
+maxDeltaT 1;
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/damBreakPermeable/system/decomposeParDict b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/system/decomposeParDict
new file mode 100644
index 0000000000000000000000000000000000000000..d96083400d61168c382b569cc2bc91911727531b
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/system/decomposeParDict
@@ -0,0 +1,27 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2012 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object decomposeParDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains 4;
+
+method simple;
+
+coeffs
+{
+ n (2 2 1);
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/damBreakPermeable/system/fvSchemes b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/system/fvSchemes
new file mode 100644
index 0000000000000000000000000000000000000000..69508dc40446828a434ae7a7c5f59633eb9a85c5
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/system/fvSchemes
@@ -0,0 +1,53 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2012 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ 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(rhoPhi,k) Gauss upwind;
+ div(rhoPhi,epsilon) Gauss upwind;
+ 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/interFoam/laminar/damBreakPermeable/system/fvSolution b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/system/fvSolution
new file mode 100644
index 0000000000000000000000000000000000000000..98dda729681a9b5d60e686dc05338c9cd7a40e6e
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/system/fvSolution
@@ -0,0 +1,83 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2012 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+ "alpha.water.*"
+ {
+ nAlphaCorr 2;
+ nAlphaSubCycles 1;
+ cAlpha 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
+ {
+ solver PCG;
+ preconditioner DIC;
+ tolerance 1e-07;
+ relTol 0.05;
+ }
+
+ p_rghFinal
+ {
+ $p_rgh;
+ relTol 0;
+ }
+
+ "(U|k|epsilon).*"
+ {
+ solver smoothSolver;
+ smoother symGaussSeidel;
+ tolerance 1e-06;
+ relTol 0;
+ minIter 1;
+ }
+}
+
+PIMPLE
+{
+ momentumPredictor no;
+ nOuterCorrectors 1;
+ nCorrectors 3;
+ nNonOrthogonalCorrectors 0;
+}
+
+relaxationFactors
+{
+ equations
+ {
+ ".*" 1;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/laminar/damBreakPermeable/system/setFieldsDict b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/system/setFieldsDict
new file mode 100644
index 0000000000000000000000000000000000000000..bb00ea228479519fa0a210160a278074a996f21f
--- /dev/null
+++ b/tutorials/multiphase/interFoam/laminar/damBreakPermeable/system/setFieldsDict
@@ -0,0 +1,35 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2012 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object setFieldsDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+defaultFieldValues
+(
+ volScalarFieldValue alpha.water 0
+);
+
+regions
+(
+ boxToCell
+ {
+ box (0 0 -1) (0.2461 0.292 1);
+ fieldValues
+ (
+ volScalarFieldValue alpha.water 1
+ );
+ }
+);
+
+
+// ************************************************************************* //