diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/U b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/U
new file mode 100644
index 0000000000000000000000000000000000000000..a719c0b5a7969de65ddf1aea1765cc2b44b9008d
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/U
@@ -0,0 +1,37 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2106 |
+| \\ / 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
+{
+ metalSheet
+ {
+ type movingWallVelocity;
+ value uniform (0 0 0);
+ }
+
+ "side-.*"
+ {
+ type pressureInletOutletVelocity;
+ value uniform (0 0 0);
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/alpha.water b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/alpha.water
new file mode 100644
index 0000000000000000000000000000000000000000..a1db4410f6f039ffc1bf623c24e3fe83b16e647d
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/alpha.water
@@ -0,0 +1,45 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2106 |
+| \\ / 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
+{
+ metalSheet
+ {
+ type zeroGradient;
+ }
+
+ "(side-01|side-06|side-03|side-04|side-05)"
+ {
+ type variableHeightFlowRate;
+ lowerBound 0;
+ upperBound 1;
+ value uniform 0;
+ }
+
+ side-02
+ {
+ type inletOutlet;
+ inletValue uniform 0;
+ value uniform 0;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/electricPotential:V b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/electricPotential:V
new file mode 100644
index 0000000000000000000000000000000000000000..e8ddde9aafdccbe2e1042d3d858c30ea369524e6
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/electricPotential:V
@@ -0,0 +1,68 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2106 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ object electricPotential:V;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [1 2 -3 0 0 -1 0];
+
+internalField uniform 0;
+
+boundaryField
+{
+ metalSheet
+ {
+ // Mandatory entries
+ type electrostaticDeposition;
+ h uniform 0;
+ CoulombicEfficiency uniform 2.14e-08;
+ resistivity uniform 3.00e+06;
+
+ // Conditional mandatory entries
+ phases
+ {
+ alpha.air
+ {
+ sigma 1e-10;
+ }
+ alpha.water
+ {
+ sigma 0.14;
+ }
+ }
+
+ // Optional entries
+ jMin 0;
+ qMin 0;
+ Rbody 0.1;
+ Vi 0;
+ qCumulative uniform 0;
+
+ // Inherited entries
+ value uniform 0;
+ }
+
+ "side-05"
+ {
+ type fixedValue;
+ value uniform 100;
+ }
+
+ "(side-01|side-02|side-03|side-04|side-06)"
+ {
+ type zeroGradient;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/k b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/k
new file mode 100644
index 0000000000000000000000000000000000000000..1aa5e1a38ce4e0112976578ba55a85588bc9e6cb
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/k
@@ -0,0 +1,38 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2106 |
+| \\ / 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 1e-3;
+
+boundaryField
+{
+ metalSheet
+ {
+ type kqRWallFunction;
+ value $internalField;
+ }
+
+ "side-.*"
+ {
+ type inletOutlet;
+ inletValue uniform 1e-3;
+ value uniform 1e-3;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/nut b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/nut
new file mode 100644
index 0000000000000000000000000000000000000000..171d330cf4e0562de0b7eae133442c21433662d6
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/nut
@@ -0,0 +1,37 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2106 |
+| \\ / 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 1e-05;
+
+boundaryField
+{
+ metalSheet
+ {
+ type nutkWallFunction;
+ value $internalField;
+ }
+
+ "side-.*"
+ {
+ type calculated;
+ value $internalField;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/omega b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/omega
new file mode 100644
index 0000000000000000000000000000000000000000..db89c49f33f1f4e48bad32850f21da329e06918a
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/omega
@@ -0,0 +1,38 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2106 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ object omega;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 0 -1 0 0 0 0];
+
+internalField uniform 0.22;
+
+boundaryField
+{
+ metalSheet
+ {
+ type omegaWallFunction;
+ value $internalField;
+ }
+
+ "side-.*"
+ {
+ type inletOutlet;
+ inletValue $internalField;
+ value $internalField;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/p_rgh b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/p_rgh
new file mode 100644
index 0000000000000000000000000000000000000000..23afaea8a2837aa2e551fee4587cf3bf3fcef670
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/0.orig/p_rgh
@@ -0,0 +1,37 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2106 |
+| \\ / 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
+{
+ metalSheet
+ {
+ type fixedFluxPressure;
+ value $internalField;
+ }
+
+ "side-.*"
+ {
+ type totalPressure;
+ p0 uniform 0;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/Allclean b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/Allclean
new file mode 100755
index 0000000000000000000000000000000000000000..fb1f3847301c377e02e12439ba58cbf303af3ef9
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/Allclean
@@ -0,0 +1,8 @@
+#!/bin/sh
+cd "${0%/*}" || exit # Run from this directory
+. ${WM_PROJECT_DIR:?}/bin/tools/CleanFunctions # Tutorial clean functions
+#------------------------------------------------------------------------------
+
+cleanCase0
+
+#------------------------------------------------------------------------------
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/Allrun b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/Allrun
new file mode 100755
index 0000000000000000000000000000000000000000..78d5debbe7f687177b9c06cd6b65b939d99f8820
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/Allrun
@@ -0,0 +1,10 @@
+#!/bin/sh
+cd "${0%/*}" || exit # Run from this directory
+. ${WM_PROJECT_DIR:?}/bin/tools/RunFunctions # Tutorial run functions
+#------------------------------------------------------------------------------
+
+./Allrun.pre
+
+runApplication $(getApplication)
+
+#------------------------------------------------------------------------------
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/Allrun-parallel b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/Allrun-parallel
new file mode 100755
index 0000000000000000000000000000000000000000..c6ef1e77d72408d756a0f2f3e11373156f6a8100
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/Allrun-parallel
@@ -0,0 +1,29 @@
+#!/bin/sh
+cd "${0%/*}" || exit # Run from this directory
+. ${WM_PROJECT_DIR:?}/bin/tools/RunFunctions # Tutorial run functions
+#------------------------------------------------------------------------------
+
+./Allrun.pre
+
+runApplication decomposePar
+
+runParallel -s 1 $(getApplication)
+
+runApplication reconstructPar
+
+
+# restart
+
+latestTime=$(foamListTimes -latestTime)
+
+mv -f "$latestTime" "$latestTime".bak
+
+rm -rf processor*
+
+runParallel -s decompose redistributePar -decompose -latestTime
+
+runParallel -s 2 $(getApplication)
+
+runParallel -s reconstruct redistributePar -reconstruct -latestTime
+
+#------------------------------------------------------------------------------
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/Allrun.pre b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/Allrun.pre
new file mode 100755
index 0000000000000000000000000000000000000000..838bd0b7b9bfbfa7a1d266a7f6c99a46834bc69d
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/Allrun.pre
@@ -0,0 +1,20 @@
+#!/bin/sh
+cd "${0%/*}" || exit # Run from this directory
+. ${WM_PROJECT_DIR:?}/bin/tools/RunFunctions # Tutorial run functions
+#------------------------------------------------------------------------------
+
+runApplication blockMesh
+
+runApplication snappyHexMesh -overwrite
+
+rm -rf 0/
+
+restore0Dir
+
+runApplication setFields
+
+runApplication transformPoints -rollPitchYaw "(0 -90 0)"
+
+runApplication checkMesh -allGeometry -allTopology
+
+#------------------------------------------------------------------------------
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/dynamicMeshDict b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/dynamicMeshDict
new file mode 100644
index 0000000000000000000000000000000000000000..2c81b3b60b44d0197501293038ac83a3a498441f
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/dynamicMeshDict
@@ -0,0 +1,28 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2106 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object dynamicMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dynamicFvMesh dynamicMotionSolverFvMesh;
+
+motionSolver solidBody;
+
+solidBodyMotionFunction tabulated6DoFMotion;
+
+timeDataFileName "<constant>/meshMotion.dat";
+
+CofG (0 0 0);
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/g b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/g
new file mode 100644
index 0000000000000000000000000000000000000000..692f4b237c97f1b89eef486f7f158ab0953ab0a6
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/g
@@ -0,0 +1,21 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2106 |
+| \\ / 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 0 -9.81);
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/hRef b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/hRef
new file mode 100644
index 0000000000000000000000000000000000000000..c776b062f3d6d1693ef76bf38f8e9a694f30abd0
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/hRef
@@ -0,0 +1,21 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2106 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class uniformDimensionedScalarField;
+ object hRef;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 1 0 0 0 0 0];
+value -0.3;
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/meshMotion.dat b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/meshMotion.dat
new file mode 100644
index 0000000000000000000000000000000000000000..67db1ba7f794c1e176a21591b7b4bb26fd985ef9
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/meshMotion.dat
@@ -0,0 +1,9 @@
+4
+(
+ // Time Linear (xyz) Rotation (xyz)
+ (0 ((0 0 0) (0 0 0)))
+ (10 ((0 0 -0.80) (0 0 0)))
+ (11 ((0 0 -0.80) (0 0 0)))
+ (21 ((0 0 0) (0 0 0)))
+)
+
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/transportProperties b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/transportProperties
new file mode 100644
index 0000000000000000000000000000000000000000..b2a79d68961cacee82fe6da8005adfc692fcba5a
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/transportProperties
@@ -0,0 +1,36 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2106 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object transportProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+phases (water air);
+
+water
+{
+ transportModel Newtonian;
+ rho 997.561;
+ nu 8.90883e-07;
+}
+
+air
+{
+ transportModel Newtonian;
+ rho 1.1765;
+ nu 1.58e-05;
+}
+
+sigma 0.072;
+
+
+// ************************************************************************* //
\ No newline at end of file
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/triSurface/metalSheet.stl.gz b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/triSurface/metalSheet.stl.gz
new file mode 100644
index 0000000000000000000000000000000000000000..10b6d02eb5bedd34900df612b7c6fb29394b4719
Binary files /dev/null and b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/triSurface/metalSheet.stl.gz differ
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/turbulenceProperties b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/turbulenceProperties
new file mode 100644
index 0000000000000000000000000000000000000000..37d673336ffebb5f886743badc79723fabec8453
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/constant/turbulenceProperties
@@ -0,0 +1,25 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2106 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object turbulenceProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType RAS;
+
+RAS
+{
+ RASModel kOmegaSST;
+}
+
+
+// ************************************************************************* //
\ No newline at end of file
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/FOelectricPotential b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/FOelectricPotential
new file mode 100644
index 0000000000000000000000000000000000000000..f75cd15be58ed7cb02f530d64fb3434516713beb
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/FOelectricPotential
@@ -0,0 +1,52 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2107 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object FOelectricPotential;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+electricPotential
+{
+ // Mandatory entries
+ type electricPotential;
+ libs (solverFunctionObjects);
+ phases
+ {
+ alpha.air
+ {
+ epsilonr 1.12940906737;
+ sigma 1e-10;
+ }
+ alpha.water
+ {
+ epsilonr 3.38822720212;
+ sigma 0.14;
+ }
+ }
+
+ // Optional entries
+ nCorr 1;
+ writeDerivedFields true;
+
+ // Inherited entries
+ region region0;
+ enabled true;
+ log true;
+ timeStart 0;
+ timeEnd 100;
+ executeControl timeStep;
+ executeInterval 1;
+ writeControl outputTime;
+ writeInterval -1;
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/blockMeshDict b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/blockMeshDict
new file mode 100644
index 0000000000000000000000000000000000000000..a5fc076502a10766742744cae4769e1a7d46d79c
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/blockMeshDict
@@ -0,0 +1,93 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2106 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+scale 0.001;
+
+vertices
+(
+ ( -1000 -500 -500 )
+ ( 1000 -500 -500 )
+ ( 1000 500 -500 )
+ ( -1000 500 -500 )
+ ( -1000 -500 500 )
+ ( 1000 -500 500 )
+ ( 1000 500 500 )
+ ( -1000 500 500 )
+);
+
+blocks
+(
+ hex (0 1 2 3 4 5 6 7) ( 40 15 15 ) simpleGrading ( 1 1 1 )
+);
+
+edges
+(
+);
+
+boundary
+(
+ side-01
+ {
+ type patch;
+ faces
+ (
+ (0 4 7 3)
+ );
+ }
+ side-02
+ {
+ type patch;
+ faces
+ (
+ (1 2 6 5)
+ );
+ }
+ side-03
+ {
+ type patch;
+ faces
+ (
+ (0 1 5 4)
+ );
+ }
+ side-04
+ {
+ type patch;
+ faces
+ (
+ (3 7 6 2)
+ );
+ }
+ side-05
+ {
+ type patch;
+ faces
+ (
+ (0 3 2 1)
+ );
+ }
+ side-06
+ {
+ type patch;
+ faces
+ (
+ (4 5 6 7)
+ );
+ }
+);
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/controlDict b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/controlDict
new file mode 100644
index 0000000000000000000000000000000000000000..0f378b1e3a62c3f1c3b3dee2ffa1615af3b0aae3
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/controlDict
@@ -0,0 +1,68 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2106 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application interFoam;
+
+startFrom latestTime;
+
+startTime 0;
+
+stopAt endTime;
+
+endTime 20;
+
+deltaT 0.001;
+
+writeControl adjustableRunTime;
+
+writeInterval 0.5;
+
+purgeWrite 0;
+
+writeFormat ascii;
+
+writePrecision 12;
+
+writeCompression off;
+
+timeFormat general;
+
+timePrecision 6;
+
+runTimeModifiable yes;
+
+adjustTimeStep yes;
+
+maxCo 10;
+
+maxAlphaCo 20;
+
+maxDeltaT 0.05;
+
+functions
+{
+ #include "FOelectricPotential"
+
+ fieldMinMax1
+ {
+ type fieldMinMax;
+ libs (fieldFunctionObjects);
+ fields ("electricPotential:V");
+ }
+}
+
+
+// ************************************************************************* //
\ No newline at end of file
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/decomposeParDict b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/decomposeParDict
new file mode 100644
index 0000000000000000000000000000000000000000..d505ad3bad801ef7bdae3c4dba2fb6a1bf6c7190
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/decomposeParDict
@@ -0,0 +1,27 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2106 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object decomposeParDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains 4;
+
+method hierarchical;
+
+coeffs
+{
+ n (4 1 1);
+}
+
+
+// ************************************************************************* //
\ No newline at end of file
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/fvSchemes b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/fvSchemes
new file mode 100644
index 0000000000000000000000000000000000000000..e4ffa606187f8fb8a4ba9ac923ef34230a34e794
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/fvSchemes
@@ -0,0 +1,60 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2106 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+ default Euler;
+}
+
+gradSchemes
+{
+ default cellLimited leastSquares 1;
+}
+
+divSchemes
+{
+ default Gauss linear;
+ div(rhoPhi,U) Gauss upwind;
+ div(phi,alpha) Gauss vanLeer;
+ div(phirb,alpha) Gauss linear;
+ div(phi,k) Gauss upwind;
+ div(phi,omega) Gauss upwind;
+ div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
+}
+
+laplacianSchemes
+{
+ default Gauss linear orthogonal;
+ laplacian(electricPotential:sigma,electricPotential:V) Gauss linear orthogonal;
+}
+
+interpolationSchemes
+{
+ default linear;
+}
+
+snGradSchemes
+{
+ default corrected;
+}
+
+wallDist
+{
+ method meshWave;
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/fvSolution b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/fvSolution
new file mode 100644
index 0000000000000000000000000000000000000000..dee59e5a28a155270eefa4765bc4c36679637804
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/fvSolution
@@ -0,0 +1,118 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2106 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+ "alpha.water.*"
+ {
+ nAlphaCorr 2;
+ nAlphaSubCycles 2;
+ cAlpha 0.8;
+ icAlpha 0;
+
+ MULESCorr yes;
+ nLimiterIter 15;
+ alphaApplyPrevCorr no;
+
+ solver smoothSolver;
+ smoother symGaussSeidel;
+ tolerance 1e-10;
+ relTol 0;
+ minIter 1;
+ }
+
+ "pcorr.*"
+ {
+ solver GAMG;
+ smoother DIC;
+ tolerance 1e-3;
+ relTol 0;
+ };
+
+ p_rgh
+ {
+ solver GAMG;
+ smoother DIC;
+ tolerance 5e-8;
+ relTol 0.01;
+ };
+
+ p_rghFinal
+ {
+ $p_rgh;
+ relTol 0;
+ }
+
+ "(U|k|omega)"
+ {
+ solver smoothSolver;
+ smoother symGaussSeidel;
+ nSweeps 1;
+ tolerance 1e-7;
+ relTol 0.1;
+ minIter 1;
+ };
+
+ "(U|k|omega)Final"
+ {
+ solver smoothSolver;
+ smoother symGaussSeidel;
+ nSweeps 1;
+ tolerance 1e-7;
+ relTol 0;
+ minIter 1;
+ };
+
+ "electricPotential:V"
+ {
+ solver PBiCGStab;
+ preconditioner DIC;
+ tolerance 1e-12;
+ relTol 0;
+ }
+}
+
+PIMPLE
+{
+ momentumPredictor no;
+
+ nOuterCorrectors 1;
+ nCorrectors 3;
+ nNonOrthogonalCorrectors 1;
+
+ correctPhi no;
+ moveMeshOuterCorrectors no;
+ turbOnFinalIterOnly yes;
+ pRefCell 0;
+ pRefValue 0;
+}
+
+relaxationFactors
+{
+ equations
+ {
+ ".*" 1;
+ "electricPotential:V" 0.5;
+ }
+}
+
+cache
+{
+ grad(U);
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/meshQualityDict b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/meshQualityDict
new file mode 100644
index 0000000000000000000000000000000000000000..8bbd4170b1de245baf58d385e16c2c1b4b19935a
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/meshQualityDict
@@ -0,0 +1,21 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2106 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object meshQualityDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+// Include defaults parameters from master dictionary
+#includeEtc "caseDicts/meshQualityDict"
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/setFieldsDict b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/setFieldsDict
new file mode 100644
index 0000000000000000000000000000000000000000..bc53d9abc56081cba2a63225fcecfa09e7dc3226
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/setFieldsDict
@@ -0,0 +1,35 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2106 |
+| \\ / 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 (-1 -1 -1) (-0.3 1 1);
+ fieldValues
+ (
+ volScalarFieldValue alpha.water 1
+ );
+ }
+);
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/snappyHexMeshDict b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/snappyHexMeshDict
new file mode 100644
index 0000000000000000000000000000000000000000..ccd942bb93d67cad1260be1bf331ec489ecf4c36
--- /dev/null
+++ b/tutorials/multiphase/interFoam/RAS/electrostaticDeposition/system/snappyHexMeshDict
@@ -0,0 +1,150 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: v2106 |
+| \\ / A nd | Website: www.openfoam.com |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object snappyHexMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+castellatedMesh true;
+snap true;
+addLayers false;
+
+geometry
+{
+ metalSheet.stl
+ {
+ type triSurfaceMesh;
+ name metalSheet;
+ }
+};
+
+castellatedMeshControls
+{
+ maxLocalCells 200000000;
+ maxGlobalCells 300000000;
+ minRefinementCells 0;
+ nCellsBetweenLevels 5;
+ maxLoadUnbalance 0.2;
+ allowFreeStandingZoneFaces false;
+ resolveFeatureAngle 1;
+
+ features
+ (
+ );
+
+ refinementSurfaces
+ {
+ metalSheet
+ {
+ level (3 3);
+ }
+ }
+
+ refinementRegions
+ {
+ metalSheet
+ {
+ mode distance;
+ levels ((0.05 3) (0.1 2));
+ }
+ }
+
+ locationInMesh ( 0.8 0 0 ) ;
+}
+
+snapControls
+{
+ tolerance 1;
+ implicitFeatureSnap true;
+ explicitFeatureSnap false;
+ multiRegionFeatureSnap false;
+ detectNearSurfacesSnap true;
+ nSmoothPatch 3;
+ nSolveIter 30;
+ nRelaxIter 5;
+ nFeatureSnapIter 5;
+ strictRegionSnap true;
+}
+
+addLayersControls
+{
+ layers
+ {
+ }
+ relativeSizes true ;
+ expansionRatio 1.2 ;
+ firstLayerThickness 0.1 ;
+ featureAngle 85;
+ slipFeatureAngle 30;
+ nGrow 0;
+ nBufferCellsNoExtrude 0;
+ minMedianAxisAngle 90;
+ maxFaceThicknessRatio 0.2;
+ maxThicknessToMedialRatio 0.3;
+ minThickness 1e-06;
+ nLayerIter 50;
+ nRelaxIter 5;
+ nSmoothSurfaceNormals 10;
+ nSmoothNormals 3;
+ nSmoothThickness 10;
+ nRelaxedIter 10;
+ nMedialAxisIter 10;
+}
+
+meshQualityControls
+{
+ minVol 1e-13;
+ minTetQuality 1e-13;
+ minArea 1e-13;
+ minTwist 0.05;
+ minDeterminant 1e-06;
+ minFaceWeight 0.02;
+ minVolRatio 0.01;
+ minTriangleTwist 0.01;
+ minFlatness 0.5;
+ maxNonOrtho 60;
+ maxBoundarySkewness 20;
+ maxInternalSkewness 4;
+ maxConcave 80;
+ nSmoothScale 4;
+ errorReduction 0.75;
+
+ relaxed
+ {
+ minVol 1e-15;
+ minTetQuality 1e-15;
+ minArea 1e-15;
+ minTwist 0.001;
+ minDeterminant 1e-06;
+ minFaceWeight 1e-06;
+ minVolRatio 0.01;
+ minTriangleTwist 0.01;
+ minFlatness 0.5;
+ maxNonOrtho 65;
+ maxBoundarySkewness 20;
+ maxInternalSkewness 4;
+ maxConcave 80;
+ nSmoothScale 4;
+ errorReduction 0.75;
+ }
+}
+
+mergeTolerance 1e-08;
+debug 0;
+
+writeFlags
+(
+ scalarLevels
+);
+
+
+// ************************************************************************* //
\ No newline at end of file