From 34bc9cadb0167f35be1cd1b656dc86b850dfc005 Mon Sep 17 00:00:00 2001
From: Henry <Henry>
Date: Sat, 1 Feb 2014 17:14:35 +0000
Subject: [PATCH] DTCHull: new interDyMFoam tutorial
---
.../interDyMFoam/ras/DTCHull/0.org/U | 58 ++++
.../ras/DTCHull/0.org/alpha.water | 54 ++++
.../interDyMFoam/ras/DTCHull/0.org/k | 54 ++++
.../interDyMFoam/ras/DTCHull/0.org/nut | 53 ++++
.../interDyMFoam/ras/DTCHull/0.org/omega | 56 ++++
.../interDyMFoam/ras/DTCHull/0.org/p_rgh | 57 ++++
.../ras/DTCHull/0.org/pointDisplacement | 52 ++++
.../interDyMFoam/ras/DTCHull/Allclean | 17 ++
.../interDyMFoam/ras/DTCHull/Allrun | 48 +++
.../ras/DTCHull/constant/RASProperties | 25 ++
.../ras/DTCHull/constant/dynamicMeshDict | 67 +++++
.../interDyMFoam/ras/DTCHull/constant/g | 21 ++
.../DTCHull/constant/polyMesh/blockMeshDict | 147 +++++++++
.../ras/DTCHull/constant/transportProperties | 36 +++
.../ras/DTCHull/constant/triSurface/README | 4 +
.../ras/DTCHull/constant/turbulenceProperties | 21 ++
.../ras/DTCHull/system/controlDict | 72 +++++
.../ras/DTCHull/system/decomposeParDict | 58 ++++
.../interDyMFoam/ras/DTCHull/system/fvSchemes | 63 ++++
.../ras/DTCHull/system/fvSolution | 117 ++++++++
.../ras/DTCHull/system/meshQualityDict | 86 ++++++
.../ras/DTCHull/system/refineMeshDict | 43 +++
.../ras/DTCHull/system/setFieldsDict | 49 +++
.../ras/DTCHull/system/snappyHexMeshDict | 284 ++++++++++++++++++
.../DTCHull/system/surfaceFeatureExtractDict | 48 +++
.../ras/DTCHull/system/topoSetDict.1 | 32 ++
.../ras/DTCHull/system/topoSetDict.2 | 32 ++
.../ras/DTCHull/system/topoSetDict.3 | 32 ++
.../ras/DTCHull/system/topoSetDict.4 | 32 ++
.../ras/DTCHull/system/topoSetDict.5 | 32 ++
.../ras/DTCHull/system/topoSetDict.6 | 32 ++
31 files changed, 1782 insertions(+)
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/U
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/alpha.water
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/k
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/nut
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/omega
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/p_rgh
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/pointDisplacement
create mode 100755 tutorials/multiphase/interDyMFoam/ras/DTCHull/Allclean
create mode 100755 tutorials/multiphase/interDyMFoam/ras/DTCHull/Allrun
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/RASProperties
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/dynamicMeshDict
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/g
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/polyMesh/blockMeshDict
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/transportProperties
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/triSurface/README
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/turbulenceProperties
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/system/controlDict
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/system/decomposeParDict
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/system/fvSchemes
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/system/fvSolution
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/system/meshQualityDict
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/system/refineMeshDict
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/system/setFieldsDict
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/system/snappyHexMeshDict
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/system/surfaceFeatureExtractDict
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.1
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.2
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.3
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.4
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.5
create mode 100644 tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.6
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/U b/tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/U
new file mode 100644
index 00000000000..507cfa947df
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/U
@@ -0,0 +1,58 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: dev |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volVectorField;
+ location "0";
+ object U;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+Umean 1.668;
+mUmean -1.668;
+
+dimensions [0 1 -1 0 0 0 0];
+
+internalField uniform ($mUmean 0 0);
+
+boundaryField
+{
+ //- Set patchGroups for constraint patches
+ #include "${WM_PROJECT_DIR}/etc/caseDicts/setConstraintTypes"
+
+ inlet
+ {
+ type fixedValue;
+ value $internalField;
+ }
+
+ outlet
+ {
+ type outletPhaseMeanVelocity;
+ alpha alpha.water;
+ Umean $Umean;
+ value $internalField;
+ }
+
+ atmosphere
+ {
+ type pressureInletOutletVelocity;
+ value uniform (0 0 0);
+ }
+
+ hull
+ {
+ type movingWallVelocity;
+ value uniform (0 0 0);
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/alpha.water b/tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/alpha.water
new file mode 100644
index 00000000000..06ee368c9c4
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/alpha.water
@@ -0,0 +1,54 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: dev |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object alpha;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 0 0 0 0 0 0];
+
+internalField uniform 0;
+
+boundaryField
+{
+ //- Set patchGroups for constraint patches
+ #include "${WM_PROJECT_DIR}/etc/caseDicts/setConstraintTypes"
+
+ inlet
+ {
+ type fixedValue;
+ value $internalField;
+ }
+
+ outlet
+ {
+ type variableHeightFlowRate;
+ lowerBound 0;
+ upperBound 1;
+ value $internalField;
+ }
+
+ atmosphere
+ {
+ type inletOutlet;
+ inletValue $internalField;
+ value $internalField;
+ }
+
+ hull
+ {
+ type zeroGradient;
+ }
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/k b/tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/k
new file mode 100644
index 00000000000..392241cd6fa
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/k
@@ -0,0 +1,54 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: dev |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object k;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 2 -2 0 0 0 0];
+
+internalField uniform 0.00015;
+
+boundaryField
+{
+ //- Set patchGroups for constraint patches
+ #include "${WM_PROJECT_DIR}/etc/caseDicts/setConstraintTypes"
+
+ inlet
+ {
+ type fixedValue;
+ value $internalField;
+ }
+
+ outlet
+ {
+ type inletOutlet;
+ inletValue $internalField;
+ value $internalField;
+ }
+
+ atmosphere
+ {
+ type inletOutlet;
+ inletValue $internalField;
+ value $internalField;
+ }
+
+ hull
+ {
+ type kqRWallFunction;
+ value $internalField;
+ }
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/nut b/tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/nut
new file mode 100644
index 00000000000..4abe529d46d
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/nut
@@ -0,0 +1,53 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: dev |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object nut;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 2 -1 0 0 0 0];
+
+internalField uniform 5e-07;
+
+boundaryField
+{
+ //- Set patchGroups for constraint patches
+ #include "${WM_PROJECT_DIR}/etc/caseDicts/setConstraintTypes"
+
+ inlet
+ {
+ type fixedValue;
+ value $internalField;
+ }
+
+ outlet
+ {
+ type zeroGradient;
+ }
+
+ atmosphere
+ {
+ type zeroGradient;
+ }
+
+ hull
+ {
+ type nutkRoughWallFunction;
+ Ks uniform 100e-6;
+ Cs uniform 0.5;
+ value $internalField;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/omega b/tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/omega
new file mode 100644
index 00000000000..0dde05c3ac1
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/omega
@@ -0,0 +1,56 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: dev |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object omega;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 0 -1 0 0 0 0];
+
+internalField uniform 2;
+
+boundaryField
+{
+ //- Set patchGroups for constraint patches
+ #include "${WM_PROJECT_DIR}/etc/caseDicts/setConstraintTypes"
+
+ inlet
+ {
+ type fixedValue;
+ value $internalField;
+ }
+
+ outlet
+ {
+ type inletOutlet;
+ inletValue $internalField;
+ value $internalField;
+ }
+
+ atmosphere
+ {
+ type inletOutlet;
+ inletValue $internalField;
+ value $internalField;
+ }
+
+ hull
+ {
+ type omegaWallFunction;
+ value $internalField;
+ }
+}
+
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/p_rgh b/tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/p_rgh
new file mode 100644
index 00000000000..0c0eda7c6fa
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/p_rgh
@@ -0,0 +1,57 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: dev |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object p_rgh;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [1 -1 -2 0 0 0 0];
+
+internalField uniform 0;
+
+boundaryField
+{
+ //- Set patchGroups for constraint patches
+ #include "${WM_PROJECT_DIR}/etc/caseDicts/setConstraintTypes"
+
+ inlet
+ {
+ type fixedFluxPressure;
+ value $internalField;
+ }
+
+ outlet
+ {
+ type zeroGradient;
+ }
+
+ atmosphere
+ {
+ type totalPressure;
+ p0 uniform 0;
+ U U;
+ phi phi;
+ rho rho;
+ psi none;
+ gamma 1;
+ value $internalField;
+ }
+
+ hull
+ {
+ type fixedFluxPressure;
+ value $internalField;
+ }
+}
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/pointDisplacement b/tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/pointDisplacement
new file mode 100644
index 00000000000..350676e605b
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/pointDisplacement
@@ -0,0 +1,52 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: dev |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class pointVectorField;
+ location "0";
+ object pointDisplacement;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 1 0 0 0 0 0];
+
+internalField uniform (0 0 0);
+
+boundaryField
+{
+ //- Set patchGroups for constraint patches
+ #include "${WM_PROJECT_DIR}/etc/caseDicts/setConstraintTypes"
+
+ inlet
+ {
+ type fixedValue;
+ value uniform (0 0 0);
+ }
+
+ outlet
+ {
+ type fixedValue;
+ value uniform (0 0 0);
+ }
+
+ atmosphere
+ {
+ type fixedValue;
+ value uniform (0 0 0);
+ }
+
+ hull
+ {
+ type calculated;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/Allclean b/tutorials/multiphase/interDyMFoam/ras/DTCHull/Allclean
new file mode 100755
index 00000000000..7ae6e656d7b
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/Allclean
@@ -0,0 +1,17 @@
+#!/bin/sh
+cd ${0%/*} || exit 1 # run from this directory
+
+# Source tutorial clean functions
+. $WM_PROJECT_DIR/bin/tools/CleanFunctions
+
+# remove surface
+\rm -f constant/triSurface/DTC-scaled.stl.gz > /dev/null 2>&1
+\rm -rf constant/extendedFeatureEdgeMesh > /dev/null 2>&1
+\rm -f constant/triSurface/DTC-scaled.eMesh > /dev/null 2>&1
+
+cleanCase
+\rm constant/polyMesh/boundary > /dev/null 2>&1
+\rm -rf 0 > /dev/null 2>&1
+\rm system/topoSetDict > /dev/null 2>&1
+
+# ----------------------------------------------------------------- end-of-file
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/Allrun b/tutorials/multiphase/interDyMFoam/ras/DTCHull/Allrun
new file mode 100755
index 00000000000..b4f55601745
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/Allrun
@@ -0,0 +1,48 @@
+#!/bin/sh
+cd ${0%/*} || exit 1 # run from this directory
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+
+runRefineMesh ()
+{
+ echo "Running refineMesh on $PWD"
+ refineMesh -dict system/refineMeshDict -overwrite > log.refineMesh 2>&1
+}
+
+# copy DTC hull surface from resources folder
+cp $FOAM_TUTORIALS/resources/geometry/DTC-scaled.stl.gz constant/triSurface/
+
+runApplication surfaceFeatureExtract
+
+runApplication blockMesh
+
+i=1
+if [ -f log.topoSet.6 ] ; then
+ i=7
+fi
+while [ "$i" -lt 7 ] ; do
+ cp system/topoSetDict.${i} system/topoSetDict
+ runApplication topoSet
+ runRefineMesh
+ mv log.topoSet log.topoSet.$i
+ mv log.refineMesh log.refineMesh.$i
+ i=$(expr $i + 1)
+done
+
+runApplication snappyHexMesh -overwrite
+
+\rm -rf 0
+\cp -r 0.org 0
+
+runApplication setFields
+
+runApplication decomposePar
+
+runParallel renumberMesh 8 -overwrite
+
+runParallel $(getApplication) 8
+
+runApplication reconstructPar
+
+# ----------------------------------------------------------------- end-of-file
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/RASProperties b/tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/RASProperties
new file mode 100644
index 00000000000..e0e6b776a27
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/RASProperties
@@ -0,0 +1,25 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: dev |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "constant";
+ object RASProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+RASModel kOmegaSST;
+
+turbulence on;
+
+printCoeffs on;
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/dynamicMeshDict b/tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/dynamicMeshDict
new file mode 100644
index 00000000000..7e7f4969af5
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/dynamicMeshDict
@@ -0,0 +1,67 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: dev |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object dynamicMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dynamicFvMesh dynamicMotionSolverFvMesh;
+
+motionSolverLibs ("libsixDoFRigidBodyMotion.so");
+
+solver sixDoFRigidBodyMotion;
+
+sixDoFRigidBodyMotionCoeffs
+{
+ patches (hull);
+ innerDistance 0.3;
+ outerDistance 1;
+
+ centreOfMass (2.929541 0 0.2);
+ mass 412.73;
+ momentOfInertia (40 921 921);
+ rhoInf 1;
+ report on;
+ accelerationRelaxation 0.3;
+ value uniform (0 0 0);
+
+ constraints
+ {
+ zAxis
+ {
+ sixDoFRigidBodyMotionConstraint line;
+ direction (0 0 1);
+ }
+ yPlane
+ {
+ sixDoFRigidBodyMotionConstraint axis;
+ axis (0 1 0);
+ }
+ }
+
+ restraints
+ {
+ translationDamper
+ {
+ sixDoFRigidBodyMotionRestraint linearDamper;
+ coeff 8596;
+ }
+ rotationDamper
+ {
+ sixDoFRigidBodyMotionRestraint sphericalAngularDamper;
+ coeff 11586;
+ }
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/g b/tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/g
new file mode 100644
index 00000000000..a0d7102656f
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/g
@@ -0,0 +1,21 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: dev |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ 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/interDyMFoam/ras/DTCHull/constant/polyMesh/blockMeshDict b/tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/polyMesh/blockMeshDict
new file mode 100644
index 00000000000..4abd94d9818
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/polyMesh/blockMeshDict
@@ -0,0 +1,147 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.2.2 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+convertToMeters 1;
+
+vertices
+(
+ (-26 -19 -16)
+ (16 -19 -16)
+ (16 0 -16)
+ (-26 0 -16)
+
+ (-26 -19 -1)
+ (16 -19 -1)
+ (16 0 -1)
+ (-26 0 -1)
+
+ (-26 -19 0.185)
+ (16 -19 0.185)
+ (16 0 0.185)
+ (-26 0 0.185)
+
+ (-26 -19 0.244)
+ (16 -19 0.244)
+ (16 0 0.244)
+ (-26 0 0.244)
+
+ (-26 -19 0.3)
+ (16 -19 0.3)
+ (16 0 0.3)
+ (-26 0 0.3)
+
+ (-26 -19 1.6)
+ (16 -19 1.6)
+ (16 0 1.6)
+ (-26 0 1.6)
+
+ (-26 -19 4)
+ (16 -19 4)
+ (16 0 4)
+ (-26 0 4)
+);
+
+blocks
+(
+ hex (0 1 2 3 4 5 6 7) (42 19 50) simpleGrading (1 1 0.05)
+ hex (4 5 6 7 8 9 10 11) (42 19 50) simpleGrading (1 1 1)
+ hex (8 9 10 11 12 13 14 15) (42 19 4) simpleGrading (1 1 1)
+ hex (12 13 14 15 16 17 18 19) (42 19 4) simpleGrading (1 1 1)
+ hex (16 17 18 19 20 21 22 23) (42 19 40) simpleGrading (1 1 1)
+ hex (20 21 22 23 24 25 26 27) (42 19 20) simpleGrading (1 1 5)
+);
+
+edges
+(
+);
+
+boundary
+(
+ atmosphere
+ {
+ type patch;
+ faces
+ (
+ (24 25 26 27)
+ );
+ }
+ inlet
+ {
+ type patch;
+ faces
+ (
+ (1 2 6 5)
+ (5 6 10 9)
+ (9 10 14 13)
+ (13 14 18 17)
+ (17 18 22 21)
+ (21 22 26 25)
+ );
+ }
+ outlet
+ {
+ type patch;
+ faces
+ (
+ (0 4 7 3)
+ (4 8 11 7)
+ (8 12 15 11)
+ (12 16 19 15)
+ (16 20 23 19)
+ (20 24 27 23)
+ );
+ }
+ bottom
+ {
+ type symmetryPlane;
+ faces
+ (
+ (0 3 2 1)
+ );
+ }
+ side
+ {
+ type symmetryPlane;
+ faces
+ (
+ (0 1 5 4)
+ (4 5 9 8)
+ (8 9 13 12)
+ (12 13 17 16)
+ (16 17 21 20)
+ (20 21 25 24)
+ );
+ }
+ midPlane
+ {
+ type symmetryPlane;
+ faces
+ (
+ (3 7 6 2)
+ (7 11 10 6)
+ (11 15 14 10)
+ (15 19 18 14)
+ (19 23 22 18)
+ (23 27 26 22)
+ );
+ }
+);
+
+mergePatchPairs
+(
+);
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/transportProperties b/tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/transportProperties
new file mode 100644
index 00000000000..0bfa2f19b96
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/transportProperties
@@ -0,0 +1,36 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: dev |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "constant";
+ object transportProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+phases (water air);
+
+water
+{
+ transportModel Newtonian;
+ nu nu [ 0 2 -1 0 0 0 0 ] 1.09e-06;
+ rho rho [ 1 -3 0 0 0 0 0 ] 998.8;
+}
+
+air
+{
+ transportModel Newtonian;
+ nu nu [ 0 2 -1 0 0 0 0 ] 1.48e-05;
+ rho rho [ 1 -3 0 0 0 0 0 ] 1;
+}
+
+sigma sigma [ 1 0 -2 0 0 0 0 ] 0;
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/triSurface/README b/tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/triSurface/README
new file mode 100644
index 00000000000..dbf3b73d5fc
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/triSurface/README
@@ -0,0 +1,4 @@
+Folder to house tri-surfaces
+
+The Allrun script copies the surface from the $FOAM_TUTORIALS/resources/geometry
+folder
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/turbulenceProperties b/tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/turbulenceProperties
new file mode 100644
index 00000000000..3721a46a2ea
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/turbulenceProperties
@@ -0,0 +1,21 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: dev |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "constant";
+ object turbulenceProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType RASModel;
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/controlDict b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/controlDict
new file mode 100644
index 00000000000..0af365257e4
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/controlDict
@@ -0,0 +1,72 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: dev |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application interDyMFoam;
+
+startFrom startTime;
+
+startTime 0;
+
+stopAt endTime;
+
+endTime 50;
+
+deltaT 0.0001;
+
+writeControl adjustableRunTime;
+
+writeInterval 5;
+
+purgeWrite 0;
+
+writeFormat binary;
+
+writePrecision 6;
+
+writeCompression uncompressed;
+
+timeFormat general;
+
+timePrecision 6;
+
+runTimeModifiable yes;
+
+adjustTimeStep yes;
+
+maxCo 25;
+maxAlphaCo 15;
+maxDeltaT 0.01;
+
+functions
+{
+ forces
+ {
+ type forces;
+ functionObjectLibs ( "libforces.so" );
+ patches (hull);
+ rhoInf 998.8;
+ rhoName rho;
+ UName U;
+ log on;
+ outputControl timeStep;
+ outputInterval 1;
+ CofR (2.929541 0 0.2);
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/decomposeParDict b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/decomposeParDict
new file mode 100644
index 00000000000..2f4ac2cb1a1
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/decomposeParDict
@@ -0,0 +1,58 @@
+/*---------------------------------------------------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 1.4 |
+| \\ / A nd | Web: http://www.openfoam.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+
+FoamFile
+{
+ version 2.0;
+ format ascii;
+
+ root "";
+ case "";
+ instance "";
+ local "";
+
+ class dictionary;
+ object decomposeParDict;
+}
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains 8;
+
+method scotch;
+
+simpleCoeffs
+{
+ n (2 1 1);
+ delta 0.001;
+}
+
+hierarchicalCoeffs
+{
+ n (1 1 1);
+ delta 0.001;
+ order xyz;
+}
+
+metisCoeffs
+{
+}
+
+manualCoeffs
+{
+ dataFile "";
+}
+
+distributed no;
+
+roots
+(
+);
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/fvSchemes b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/fvSchemes
new file mode 100644
index 00000000000..4bca38f8ba9
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/fvSchemes
@@ -0,0 +1,63 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: dev |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+ default Euler;
+}
+
+gradSchemes
+{
+ default Gauss linear;
+ limitedGrad cellLimited Gauss linear 1;
+}
+
+divSchemes
+{
+ div(rhoPhi,U) Gauss linearUpwind grad(U);
+ div(phi,alpha) Gauss vanLeer;
+ div(phirb,alpha) Gauss linear;
+ div(phi,k) Gauss linearUpwind limitedGrad;
+ div(phi,omega) Gauss linearUpwind limitedGrad;
+ div((muEff*dev(T(grad(U))))) Gauss linear;
+}
+
+laplacianSchemes
+{
+ default Gauss linear corrected;
+}
+
+interpolationSchemes
+{
+ default linear;
+}
+
+snGradSchemes
+{
+ default corrected;
+}
+
+fluxRequired
+{
+ default no;
+ p_rgh;
+ pcorr;
+ alpha.water;
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/fvSolution b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/fvSolution
new file mode 100644
index 00000000000..208497384fb
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/fvSolution
@@ -0,0 +1,117 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: dev |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+ "alpha.water.*"
+ {
+ nAlphaCorr 3;
+ nAlphaSubCycles 1;
+ cAlpha 1;
+ icAlpha 0;
+
+ alphaOuterCorrectors yes;
+
+ MULESCorr yes;
+ nLimiterIter 10;
+ alphaApplyPrevCorr yes;
+
+ solver smoothSolver;
+ smoother symGaussSeidel;
+ tolerance 1e-10;
+ relTol 0;
+ minIter 1;
+ }
+
+ "pcorr.*"
+ {
+ solver GAMG;
+
+ smoother DIC;
+ agglomerator faceAreaPair;
+ mergeLevels 1;
+ nCellsInCoarsestLevel 10;
+ cacheAgglomeration true;
+
+ tolerance 0.1;
+ relTol 0;
+ };
+
+ p_rgh
+ {
+ solver GAMG;
+
+ smoother DIC;
+ agglomerator faceAreaPair;
+ mergeLevels 1;
+ nCellsInCoarsestLevel 10;
+ cacheAgglomeration true;
+
+ tolerance 5e-8;
+ relTol 0.001;
+ };
+
+ p_rghFinal
+ {
+ $p_rgh;
+ relTol 0;
+ }
+
+ "(U|k|omega).*"
+ {
+ solver smoothSolver;
+
+ smoother symGaussSeidel;
+ nSweeps 1;
+
+ tolerance 1e-7;
+ relTol 0;
+ minIter 1;
+ };
+}
+
+PIMPLE
+{
+ momentumPredictor no;
+
+ nOuterCorrectors 1;
+ nCorrectors 3;
+ nNonOrthogonalCorrectors 0;
+
+ correctPhi yes;
+ moveMeshOuterCorrectors yes;
+ turbOnFinalIterOnly yes;
+}
+
+relaxationFactors
+{
+ fields
+ {
+ }
+ equations
+ {
+ ".*" 1;
+ }
+}
+
+cache
+{
+ grad(U);
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/meshQualityDict b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/meshQualityDict
new file mode 100644
index 00000000000..465d20f1c51
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/meshQualityDict
@@ -0,0 +1,86 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.2.x |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object meshQualityDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+//- Maximum non-orthogonality allowed. Set to 180 to disable.
+maxNonOrtho 70;
+
+//- Max skewness allowed. Set to <0 to disable.
+maxBoundarySkewness 20;
+maxInternalSkewness 4;
+
+//- Max concaveness allowed. Is angle (in degrees) below which concavity
+// is allowed. 0 is straight face, <0 would be convex face.
+// Set to 180 to disable.
+maxConcave 80;
+
+//- Minimum pyramid volume. Is absolute volume of cell pyramid.
+// Set to a sensible fraction of the smallest cell volume expected.
+// Set to very negative number (e.g. -1E30) to disable.
+minVol 1e-13;
+
+//- Minimum quality of the tet formed by the face-centre
+// and variable base point minimum decomposition triangles and
+// the cell centre. Set to very negative number (e.g. -1E30) to
+// disable.
+// <0 = inside out tet,
+// 0 = flat tet
+// 1 = regular tet
+minTetQuality 1e-30;
+
+//- Minimum face area. Set to <0 to disable.
+minArea -1;
+
+//- Minimum face twist. Set to <-1 to disable. dot product of face normal
+//- and face centre triangles normal
+minTwist 0.05;
+
+//- minimum normalised cell determinant
+//- 1 = hex, <= 0 = folded or flattened illegal cell
+minDeterminant 0.001;
+
+//- minFaceWeight (0 -> 0.5)
+minFaceWeight 0.05;
+
+//- minVolRatio (0 -> 1)
+minVolRatio 0.01;
+
+//must be >0 for Fluent compatibility
+minTriangleTwist -1;
+
+//- if >0 : preserve single cells with all points on the surface if the
+// resulting volume after snapping (by approximation) is larger than
+// minVolCollapseRatio times old volume (i.e. not collapsed to flat cell).
+// If <0 : delete always.
+//minVolCollapseRatio 0.5;
+
+
+// Advanced
+
+//- Number of error distribution iterations
+nSmoothScale 4;
+//- amount to scale back displacement at error points
+errorReduction 0.75;
+
+
+
+// Optional : some meshing phases allow usage of relaxed rules.
+// See e.g. addLayersControls::nRelaxedIter.
+relaxed
+{
+ //- Maximum non-orthogonality allowed. Set to 180 to disable.
+ maxNonOrtho 75;
+}
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/refineMeshDict b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/refineMeshDict
new file mode 100644
index 00000000000..9516d1cf6a6
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/refineMeshDict
@@ -0,0 +1,43 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.2.2 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object refineMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+set c0;
+
+coordinateSystem global;
+
+globalCoeffs
+{
+ tan1 ( 1 0 0 );
+ tan2 ( 0 1 0 );
+}
+
+patchLocalCoeffs
+{
+ patch outside;
+ tan1 ( 1 0 0 );
+}
+
+directions ( tan1 tan2 );
+
+useHexTopology no;
+
+geometricCut yes;
+
+writeMesh no;
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/setFieldsDict b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/setFieldsDict
new file mode 100644
index 00000000000..c19c3b991d1
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/setFieldsDict
@@ -0,0 +1,49 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: dev |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object setFieldsDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+defaultFieldValues
+(
+ volScalarFieldValue alpha.water 0
+);
+
+regions
+(
+ // Set cell values
+ // (does zerogradient on boundaries)
+ boxToCell
+ {
+ box (-999 -999 -999) (999 999 0.244);
+
+ fieldValues
+ (
+ volScalarFieldValue alpha.water 1
+ );
+ }
+
+ // Set patch values (using ==)
+ boxToFace
+ {
+ box (-999 -999 -999) (999 999 0.244);
+
+ fieldValues
+ (
+ volScalarFieldValue alpha.water 1
+ );
+ }
+);
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/snappyHexMeshDict b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/snappyHexMeshDict
new file mode 100644
index 00000000000..fbb5e12522a
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/snappyHexMeshDict
@@ -0,0 +1,284 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: dev |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object snappyHexMeshDict;
+}
+
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+// Which of the steps to run
+castellatedMesh true;
+snap true;
+addLayers true;
+
+
+// Geometry. Definition of all surfaces. All surfaces are of class
+// searchableSurface.
+// Surfaces are used
+// - to specify refinement for any mesh cell intersecting it
+// - to specify refinement for any mesh cell inside/outside/near
+// - to 'snap' the mesh boundary to the surface
+geometry
+{
+ DTC-scaled.stl
+ {
+ type triSurfaceMesh;
+ name hull;
+
+ patchInfo
+ {
+ type wall;
+ }
+ }
+};
+
+
+
+// Settings for the castellatedMesh generation.
+castellatedMeshControls
+{
+
+ // Refinement parameters
+ // ~~~~~~~~~~~~~~~~~~~~~
+
+ // If local number of cells is >= maxLocalCells on any processor
+ // switches from from refinement followed by balancing
+ // (current method) to (weighted) balancing before refinement.
+ maxLocalCells 100000;
+
+ // Overall cell limit (approximately). Refinement will stop immediately
+ // upon reaching this number so a refinement level might not complete.
+ // Note that this is the number of cells before removing the part which
+ // is not 'visible' from the keepPoint. The final number of cells might
+ // actually be a lot less.
+ maxGlobalCells 2000000;
+
+ // The surface refinement loop might spend lots of iterations refining just a
+ // few cells. This setting will cause refinement to stop if <= minimumRefine
+ // are selected for refinement. Note: it will at least do one iteration
+ // (unless the number of cells to refine is 0)
+ minRefinementCells 0;
+
+ // Number of buffer layers between different levels.
+ // 1 means normal 2:1 refinement restriction, larger means slower
+ // refinement.
+ nCellsBetweenLevels 3;
+
+
+
+ // Explicit feature edge refinement
+ // ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+
+ // Specifies a level for any cell intersected by its edges.
+ // This is a featureEdgeMesh, read from constant/triSurface for now.
+ features
+ (
+ {
+ file "DTC-scaled.eMesh";
+ level 0;
+ }
+ );
+
+
+
+ // Surface based refinement
+ // ~~~~~~~~~~~~~~~~~~~~~~~~
+
+ // Specifies two levels for every surface. The first is the minimum level,
+ // every cell intersecting a surface gets refined up to the minimum level.
+ // The second level is the maximum level. Cells that 'see' multiple
+ // intersections where the intersections make an
+ // angle > resolveFeatureAngle get refined up to the maximum level.
+
+ refinementSurfaces
+ {
+ hull
+ {
+ // Surface-wise min and max refinement level
+ level (0 0);
+ }
+ }
+
+ resolveFeatureAngle 45;
+
+
+ // Region-wise refinement
+ // ~~~~~~~~~~~~~~~~~~~~~~
+
+ // Specifies refinement level for cells in relation to a surface. One of
+ // three modes
+ // - distance. 'levels' specifies per distance to the surface the
+ // wanted refinement level. The distances need to be specified in
+ // descending order.
+ // - inside. 'levels' is only one entry and only the level is used. All
+ // cells inside the surface get refined up to the level. The surface
+ // needs to be closed for this to be possible.
+ // - outside. Same but cells outside.
+
+ refinementRegions
+ {
+ }
+
+
+ // Mesh selection
+ // ~~~~~~~~~~~~~~
+
+ // After refinement patches get added for all refinementSurfaces and
+ // all cells intersecting the surfaces get put into these patches. The
+ // section reachable from the locationInMesh is kept.
+ // NOTE: This point should never be on a face, always inside a cell, even
+ // after refinement.
+ locationInMesh (-0.7 0 0);
+
+
+ // Whether any faceZones (as specified in the refinementSurfaces)
+ // are only on the boundary of corresponding cellZones or also allow
+ // free-standing zone faces. Not used if there are no faceZones.
+ allowFreeStandingZoneFaces true;
+}
+
+
+
+// Settings for the snapping.
+snapControls
+{
+ //- Number of patch smoothing iterations before finding correspondence
+ // to surface
+ nSmoothPatch 3;
+
+ //- Relative distance for points to be attracted by surface feature point
+ // or edge. True distance is this factor times local
+ // maximum edge length.
+ // tolerance 4.0;
+ tolerance 1.0;
+
+ //- Number of mesh displacement relaxation iterations.
+ nSolveIter 100;
+
+ //- Maximum number of snapping relaxation iterations. Should stop
+ // before upon reaching a correct mesh.
+ nRelaxIter 5;
+
+ nFeatureSnapIter 10;
+}
+
+
+
+// Settings for the layer addition.
+addLayersControls
+{
+ // Are the thickness parameters below relative to the undistorted
+ // size of the refined cell outside layer (true) or absolute sizes (false).
+ relativeSizes true;
+
+ // Per final patch (so not geometry!) the layer information
+ layers
+ {
+ hull
+ {
+ nSurfaceLayers 3;
+
+ }
+ }
+
+ // Expansion factor for layer mesh
+ expansionRatio 1.5;
+
+
+ // Wanted thickness of final added cell layer. If multiple layers
+ // is the thickness of the layer furthest away from the wall.
+ // See relativeSizes parameter.
+ finalLayerThickness 0.7;
+
+ // Minimum thickness of cell layer. If for any reason layer
+ // cannot be above minThickness do not add layer.
+ // See relativeSizes parameter.
+ minThickness 0.25;
+
+ // If points get not extruded do nGrow layers of connected faces that are
+ // also not grown. This helps convergence of the layer addition process
+ // close to features.
+ // Note: changed(corrected) w.r.t 17x! (didn't do anything in 17x)
+ nGrow 0;
+
+
+ // Advanced settings
+
+ // When not to extrude surface. 0 is flat surface, 90 is when two faces
+ // are perpendicular
+ featureAngle 60;
+
+ // Maximum number of snapping relaxation iterations. Should stop
+ // before upon reaching a correct mesh.
+ nRelaxIter 5;
+
+ // Number of smoothing iterations of surface normals
+ nSmoothSurfaceNormals 1;
+
+ // Number of smoothing iterations of interior mesh movement direction
+ nSmoothNormals 3;
+
+ // Smooth layer thickness over surface patches
+ nSmoothThickness 10;
+
+ // Stop layer growth on highly warped cells
+ maxFaceThicknessRatio 0.5;
+
+ // Reduce layer growth where ratio thickness to medial
+ // distance is large
+ maxThicknessToMedialRatio 0.3;
+
+ // Angle used to pick up medial axis points
+ // Note: changed(corrected) w.r.t 17x! 90 degrees corresponds to 130 in 17x.
+ minMedianAxisAngle 90;
+
+ // Create buffer region for new layer terminations
+ nBufferCellsNoExtrude 0;
+
+
+ // Overall max number of layer addition iterations. The mesher will exit
+ // if it reaches this number of iterations; possibly with an illegal
+ // mesh.
+ nLayerIter 50;
+
+ // Max number of iterations after which relaxed meshQuality controls
+ // get used. Up to nRelaxIter it uses the settings in meshQualityControls,
+ // after nRelaxIter it uses the values in meshQualityControls::relaxed.
+ nRelaxedIter 20;
+}
+
+
+
+// Generic mesh quality settings. At any undoable phase these determine
+// where to undo.
+meshQualityControls
+{
+ #include "meshQualityDict"
+}
+
+
+// Advanced
+
+// Flags for optional output
+// 0 : only write final meshes
+// 1 : write intermediate meshes
+// 2 : write volScalarField with cellLevel for postprocessing
+// 4 : write current intersections as .obj files
+debug 0;
+
+
+// Merge tolerance. Is fraction of overall bounding box of initial mesh.
+// Note: the write tolerance needs to be higher than this.
+mergeTolerance 1E-6;
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/surfaceFeatureExtractDict b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/surfaceFeatureExtractDict
new file mode 100644
index 00000000000..bba292f5768
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/surfaceFeatureExtractDict
@@ -0,0 +1,48 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.2.2 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object surfaceFeatureExtractDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+DTC-scaled.stl
+{
+ // How to obtain raw features (extractFromFile || extractFromSurface)
+ extractionMethod extractFromSurface;
+
+ extractFromSurfaceCoeffs
+ {
+ // Mark edges whose adjacent surface normals are at an angle less
+ // than includedAngle as features
+ // - 0 : selects no edges
+ // - 180: selects all edges
+ includedAngle 150;
+ }
+
+ subsetFeatures
+ {
+ // Keep nonManifold edges (edges with >2 connected faces)
+ nonManifoldEdges yes;
+
+ // Keep open edges (edges with 1 connected face)
+ openEdges yes;
+ }
+
+
+ // Write options
+
+ // Write features to obj format for postprocessing
+ writeObj yes;
+}
+
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.1 b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.1
new file mode 100644
index 00000000000..ec5de6422dc
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.1
@@ -0,0 +1,32 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.2.2 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object topoSetDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+actions
+(
+ {
+ name c0;
+ type cellSet;
+ action new;
+ source boxToCell;
+ sourceInfo
+ {
+ box (-10 -6 -3) (10 0 3);
+ }
+ }
+);
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.2 b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.2
new file mode 100644
index 00000000000..902dd3ba3c9
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.2
@@ -0,0 +1,32 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.2.2 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object topoSetDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+actions
+(
+ {
+ name c0;
+ type cellSet;
+ action new;
+ source boxToCell;
+ sourceInfo
+ {
+ box (-5 -3 -2.5) (9 0 2);
+ }
+ }
+);
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.3 b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.3
new file mode 100644
index 00000000000..74843219116
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.3
@@ -0,0 +1,32 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.2.2 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object topoSetDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+actions
+(
+ {
+ name c0;
+ type cellSet;
+ action new;
+ source boxToCell;
+ sourceInfo
+ {
+ box (-3 -1.5 -1) (8 0 1.5);
+ }
+ }
+);
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.4 b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.4
new file mode 100644
index 00000000000..7b6fb9f99f4
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.4
@@ -0,0 +1,32 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.2.2 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object topoSetDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+actions
+(
+ {
+ name c0;
+ type cellSet;
+ action new;
+ source boxToCell;
+ sourceInfo
+ {
+ box (-2 -1 -0.6) (7 0 1);
+ }
+ }
+);
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.5 b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.5
new file mode 100644
index 00000000000..410c7b036c5
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.5
@@ -0,0 +1,32 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.2.2 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object topoSetDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+actions
+(
+ {
+ name c0;
+ type cellSet;
+ action new;
+ source boxToCell;
+ sourceInfo
+ {
+ box (-1 -0.6 -0.3) (6.5 0 0.8);
+ }
+ }
+);
+
+// ************************************************************************* //
diff --git a/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.6 b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.6
new file mode 100644
index 00000000000..81547b62340
--- /dev/null
+++ b/tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.6
@@ -0,0 +1,32 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.2.2 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object topoSetDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+actions
+(
+ {
+ name c0;
+ type cellSet;
+ action new;
+ source boxToCell;
+ sourceInfo
+ {
+ box (-0.5 -0.55 -0.15) (6.25 0 0.65);
+ }
+ }
+);
+
+// ************************************************************************* //
--
GitLab