tutorials: Examples of mapFieldsPar usage

Two pitzDaily variants have been added; pitzDailySteadyMappedToPart, and
pitzDailySteadyMappedToRefined. These demonstrate usage of workflows
which involve mapping between cases with mapFieldsPar.

The pitzDailySteadyMappedToPart case demonstrates mapping onto a small
section of the mesh; in this case in the vicinity of the the corner of
the backstep. This mesh is not consistent with the source data, so
fields are required in the zero directory and cutting patches are used
to specify the properties at the inlets.

The pitzDailySteadyMappedToRefined case demonstrates mapping onto a
geometrically similar case with a different mesh density. This mesh is
consistent with the source, so no fields are needed and no cutting
patches are used. This case does, however, perturb the geometry of the
block mesh a bit, so that some of the refined case is not overlapping
the original case. This provides a test of the stabilisation
procedures within the mesh-to-mesh mapping functions.

tutorials/modules/incompressibleFluid/pitzDailySteadyMappedToPart/0/U.orig

@@ -0,0 +1,43 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       volVectorField;
+    location    "0";
+    object      U;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 1 -1 0 0 0 0];
+
+internalField   uniform (0 0 0);
+
+boundaryField
+{
+    cutIn
+    {
+        type            fixedValue;
+        value           $internalField;
+    }
+    cutOut
+    {
+        type            pressureInletOutletVelocity;
+        value           $internalField;
+    }
+    lowerWall
+    {
+        type            noSlip;
+    }
+    frontAndBack
+    {
+        type            empty;
+    }
+}
+
+// ************************************************************************* //

tutorials/modules/incompressibleFluid/pitzDailySteadyMappedToPart/0/epsilon.orig

@@ -0,0 +1,46 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       volScalarField;
+    location    "0";
+    object      epsilon;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 2 -3 0 0 0 0];
+
+internalField   uniform 14.855;
+
+boundaryField
+{
+    cutIn
+    {
+        type            fixedValue;
+        value           $internalField;
+    }
+    cutOut
+    {
+        type            inletOutlet;
+        inletValue      $internalField;
+        value           $internalField;
+    }
+    lowerWall
+    {
+        type            epsilonWallFunction;
+        value           $internalField;
+    }
+    frontAndBack
+    {
+        type            empty;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/modules/incompressibleFluid/pitzDailySteadyMappedToPart/0/k.orig

@@ -0,0 +1,46 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       volScalarField;
+    location    "0";
+    object      k;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 2 -2 0 0 0 0];
+
+internalField   uniform 0.375;
+
+boundaryField
+{
+    cutIn
+    {
+        type            fixedValue;
+        value           $internalField;
+    }
+    cutOut
+    {
+        type            inletOutlet;
+        inletValue      $internalField;
+        value           $internalField;
+    }
+    lowerWall
+    {
+        type            kqRWallFunction;
+        value           $internalField;
+    }
+    frontAndBack
+    {
+        type            empty;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/modules/incompressibleFluid/pitzDailySteadyMappedToPart/0/nut.orig

@@ -0,0 +1,45 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       volScalarField;
+    location    "0";
+    object      nut;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 2 -1 0 0 0 0];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    cutIn
+    {
+        type            calculated;
+        value           $internalField;
+    }
+    cutOut
+    {
+        type            calculated;
+        value           $internalField;
+    }
+    lowerWall
+    {
+        type            nutkWallFunction;
+        value           $internalField;
+    }
+    frontAndBack
+    {
+        type            empty;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/modules/incompressibleFluid/pitzDailySteadyMappedToPart/0/p.orig

@@ -0,0 +1,43 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       volScalarField;
+    location    "0";
+    object      p;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 2 -2 0 0 0 0];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    cutIn
+    {
+        type            zeroGradient;
+    }
+    cutOut
+    {
+        type            entrainmentPressure;
+        p0              $internalField;
+        value           $internalField;
+    }
+    lowerWall
+    {
+        type            zeroGradient;
+    }
+    frontAndBack
+    {
+        type            empty;
+    }
+}
+
+// ************************************************************************* //

tutorials/modules/incompressibleFluid/pitzDailySteadyMappedToPart/Allclean

@@ -0,0 +1,9 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # Run from this directory
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/CleanFunctions
+
+cleanCase && rm -rf pitzDailySteady constant system/controlDict system/fv*
+
+#------------------------------------------------------------------------------

tutorials/modules/incompressibleFluid/pitzDailySteadyMappedToPart/Allrun

@@ -0,0 +1 @@
+Allrun-parallel

tutorials/modules/incompressibleFluid/pitzDailySteadyMappedToPart/Allrun-parallel

@@ -0,0 +1,46 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # Run from this directory
+
+# Source tutorial run and clean functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+. $WM_PROJECT_DIR/bin/tools/CleanFunctions
+
+# Copy the source case
+isTest "$@" && path=.. || path=$FOAM_TUTORIALS/modules/incompressibleFluid
+cp -r $path/pitzDailySteady/constant .
+cp -r $path/pitzDailySteady/system/controlDict system
+cp -r $path/pitzDailySteady/system/fv* system
+cp -r $path/pitzDailySteady .
+
+# Run the source case in parallel
+(
+    cd pitzDailySteady
+    isTest "$@" && cleanCase
+    cp ../system/decomposeParDict system
+    runApplication blockMesh -dict $FOAM_TUTORIALS/resources/blockMesh/pitzDaily
+    runApplication decomposePar
+    runParallel foamRun
+)
+
+# Mesh
+runApplication blockMesh
+runApplication decomposePar
+
+# Map from the source case into this case and run in parallel
+#
+# !!! Smooth interpolative mapping from a coarse to a fine case is not
+# available within mapFieldsPar. All current options create fields with step
+# changes at the boundaries between coarse source cells. This poor
+# initialisation results in a large transient at the start of the part
+# simulation. We need a lot of under-relaxation to overcome this. In future, it
+# is desired to introduce smooth interpolative mapping, which should resolve
+# this issue and the need for additional under-relaxation.
+#
+runParallel mapFieldsPar pitzDailySteady -sourceTime latestTime -fields "(epsilon k nut p U)"
+runApplication foamDictionary system/fvSolution -entry relaxationFactors/equations -set '{ ".*" 0.1; }'
+runParallel foamRun
+
+# Reconstruct, including the values mapped to the zero directory
+runApplication reconstructPar -withZero
+
+#------------------------------------------------------------------------------

tutorials/modules/incompressibleFluid/pitzDailySteadyMappedToPart/Allrun-serial

@@ -0,0 +1,39 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # Run from this directory
+
+# Source tutorial run and clean functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+. $WM_PROJECT_DIR/bin/tools/CleanFunctions
+
+# Copy the source case
+isTest "$@" && path=.. || path=$FOAM_TUTORIALS/modules/incompressibleFluid
+cp -r $path/pitzDailySteady/constant .
+cp -r $path/pitzDailySteady/system/controlDict system
+cp -r $path/pitzDailySteady/system/fv* system
+cp -r $path/pitzDailySteady .
+
+# Run the source case
+(
+    cd pitzDailySteady
+    isTest "$@" && cleanCase
+    ./Allrun
+)
+
+# Mesh
+runApplication blockMesh
+
+# Map from the source case into this case and run
+#
+# !!! Smooth interpolative mapping from a coarse to a fine case is not
+# available within mapFieldsPar. All current options create fields with step
+# changes at the boundaries between coarse source cells. This poor
+# initialisation results in a large transient at the start of the part
+# simulation. We need a lot of under-relaxation to overcome this. In future, it
+# is desired to introduce smooth interpolative mapping, which should resolve
+# this issue and the need for additional under-relaxation.
+#
+runApplication mapFieldsPar pitzDailySteady -sourceTime latestTime -fields "(epsilon k nut p U)"
+runApplication foamDictionary system/fvSolution -entry relaxationFactors/equations -set '{ ".*" 0.1; }'
+runApplication foamRun
+
+#------------------------------------------------------------------------------

tutorials/modules/incompressibleFluid/pitzDailySteadyMappedToPart/system/blockMeshDict

@@ -0,0 +1,85 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    object      blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+convertToMeters 0.001;
+
+vertices
+(
+    (-2 0 -0.5)
+    (-2 1 -0.5)
+    (0 -1 -0.5)
+    (0 0 -0.5)
+    (0 1 -0.5)
+    (2 -1 -0.5)
+    (2 0 -0.5)
+    (2 1 -0.5)
+
+    (-2 0 0.5)
+    (-2 1 0.5)
+    (0 -1 0.5)
+    (0 0 0.5)
+    (0 1 0.5)
+    (2 -1 0.5)
+    (2 0 0.5)
+    (2 1 0.5)
+);
+
+blocks
+(
+    hex (0 3 4 1 8 11 12 9) (30 40 1) simpleGrading (0.2 5 1)
+    hex (2 5 6 3 10 13 14 11) (30 40 1) simpleGrading (5 0.2 1)
+    hex (3 6 7 4 11 14 15 12) (30 40 1) simpleGrading (5 5 1)
+);
+
+defaultPatch
+{
+    name frontAndBack;
+    type empty;
+}
+
+boundary
+(
+    lowerWall
+    {
+        type wall;
+        faces
+        (
+            (0 3 11 8)
+            (3 2 10 11)
+        );
+    }
+    cutIn
+    {
+        type patch;
+        faces
+        (
+            (0 1 9 8)
+            (2 5 13 10)
+        );
+    }
+    cutOut
+    {
+        type patch;
+        faces
+        (
+            (1 4 12 9)
+            (4 7 15 12)
+            (5 6 14 13)
+            (6 7 15 14)
+        );
+    }
+);
+
+// ************************************************************************* //

tutorials/modules/incompressibleFluid/pitzDailySteadyMappedToPart/system/decomposeParDict

@@ -0,0 +1,20 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    object      decomposeParDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains  4;
+
+method              scotch;
+
+// ************************************************************************* //

tutorials/modules/incompressibleFluid/pitzDailySteadyMappedToPart/system/mapFieldsDict

@@ -0,0 +1,20 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    object      mapFieldsDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+patchMap        (lowerWall lowerWall);
+
+cuttingPatches  (cutIn);
+
+// ************************************************************************* //

tutorials/modules/incompressibleFluid/pitzDailySteadyMappedToRefined/Allclean

@@ -0,0 +1,11 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # Run from this directory
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/CleanFunctions
+
+cleanCase && rm -rf pitzDailySteady 0 constant
+
+find system -type f -not -name decomposeParDict -delete
+
+#------------------------------------------------------------------------------

tutorials/modules/incompressibleFluid/pitzDailySteadyMappedToRefined/Allmesh

@@ -0,0 +1,30 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # Run from this directory
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+
+# Get the standard mesh dictionary
+cp -f $FOAM_TUTORIALS/resources/blockMesh/pitzDaily system
+
+# Decrease the mesh spacings by a factor
+factor=5/4
+for nX in 18 180 25
+do
+    for nY in 27 30
+    do
+        nXYZ0="($nX $nY 1)"
+        nXYZ1="($(echo $nX*$factor | bc) $(echo $nY*$factor | bc) 1)"
+        sed -i "s/$nXYZ0/$nXYZ1/g" system/blockMeshDict
+    done
+done
+
+# Create a slightly inconsistent geometry, with some cells and patch faces
+# falling outside the source case. This tests the stabilisation of the
+# mesh-to-mesh interpolations.
+sed -i 's/(0 0 \(.*\))/(-1.2 0 \1)/g' system/blockMeshDict
+
+# Mesh
+runApplication blockMesh
+
+#------------------------------------------------------------------------------

tutorials/modules/incompressibleFluid/pitzDailySteadyMappedToRefined/Allrun

@@ -0,0 +1 @@
+Allrun-parallel

tutorials/modules/incompressibleFluid/pitzDailySteadyMappedToRefined/Allrun-parallel

@@ -0,0 +1,35 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # Run from this directory
+
+# Source tutorial run and clean functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+. $WM_PROJECT_DIR/bin/tools/CleanFunctions
+
+# Copy the source case
+isTest "$@" && path=.. || path=$FOAM_TUTORIALS/modules/incompressibleFluid
+cp -r $path/pitzDailySteady/constant .
+cp -r $path/pitzDailySteady/system/* system
+cp -r $path/pitzDailySteady .
+
+# Run the source case in parallel
+(
+    cd pitzDailySteady
+    isTest "$@" && cleanCase
+    cp ../system/decomposeParDict system
+    runApplication blockMesh -dict $FOAM_TUTORIALS/resources/blockMesh/pitzDaily
+    runApplication decomposePar
+    runParallel foamRun
+)
+
+# Mesh
+./Allmesh
+runApplication decomposePar
+
+# Map from the source case into this case and run
+runParallel mapFieldsPar pitzDailySteady -consistent -sourceTime latestTime
+runParallel foamRun
+
+# Reconstruct, including the values mapped to the zero directory
+runApplication reconstructPar -withZero
+
+#------------------------------------------------------------------------------

tutorials/modules/incompressibleFluid/pitzDailySteadyMappedToRefined/Allrun-serial

@@ -0,0 +1,28 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # Run from this directory
+
+# Source tutorial run and clean functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+. $WM_PROJECT_DIR/bin/tools/CleanFunctions
+
+# Copy the source case
+isTest "$@" && path=.. || path=$FOAM_TUTORIALS/modules/incompressibleFluid
+cp -r $path/pitzDailySteady/constant .
+cp -r $path/pitzDailySteady/system/* system
+cp -r $path/pitzDailySteady .
+
+# Run the source case
+(
+    cd pitzDailySteady
+    isTest "$@" && cleanCase
+    ./Allrun
+)
+
+# Mesh
+./Allmesh
+
+# Map from the source case into this case and run
+runApplication mapFieldsPar pitzDailySteady -consistent -sourceTime latestTime
+runApplication foamRun
+
+#------------------------------------------------------------------------------

tutorials/modules/incompressibleFluid/pitzDailySteadyMappedToRefined/system/decomposeParDict

@@ -0,0 +1,20 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    format      ascii;
+    class       dictionary;
+    object      decomposeParDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains  4;
+
+method              scotch;
+
+// ************************************************************************* //