drivaerFastback: example case of automotive aerodynamics

tutorials/incompressible/simpleFoam/drivaerFastback/0/U

@@ -0,0 +1,70 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volVectorField;
+    object      U;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+Uinlet          16;
+
+wheelRadius     0.318;
+wheelBase       2.786;
+wheelSpeed      #calc "$Uinlet / $wheelRadius";
+
+
+dimensions      [0 1 -1 0 0 0 0];
+
+internalField   uniform (0 0 0);
+
+boundaryField
+{
+    inlet
+    {
+        type            fixedValue;
+        value           uniform ($Uinlet 0 0);
+    }
+
+    ground { $inlet; }
+
+    freestream
+    {
+        type            freestreamVelocity;
+        freestreamValue uniform ($Uinlet 0 0);
+    }
+
+    wall
+    {
+        type            noSlip;
+    }
+
+    frontWheels
+    {
+        type            rotatingWallVelocity;
+        origin          (0 0 $wheelRadius);
+        axis            (0 -1 0);
+        omega           $wheelSpeed;
+    }
+
+    rearWheels
+    {
+        $frontWheels;
+        origin          ($wheelBase 0 $wheelRadius);
+    }
+
+    processor
+    {
+        type            processor;
+        value           uniform (0 0 0);
+    }
+}
+
+// ************************************************************************* //

tutorials/incompressible/simpleFoam/drivaerFastback/0/k

@@ -0,0 +1,51 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      k;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+kInlet          0.002;
+
+dimensions      [0 2 -2 0 0 0 0];
+
+internalField   uniform $kInlet;
+
+boundaryField
+{
+    inlet
+    {
+        type            fixedValue;
+        value           uniform $kInlet;
+    }
+
+    freestream
+    {
+        type            inletOutlet;
+        inletValue      uniform $kInlet;
+        value           uniform $kInlet;
+    }
+
+    wall
+    {
+        type            kqRWallFunction;
+        value           uniform $kInlet;
+    }
+
+    processor
+    {
+        type            processor;
+        value           uniform $kInlet;
+    }
+}
+
+// ************************************************************************* //

tutorials/incompressible/simpleFoam/drivaerFastback/0/nut

@@ -0,0 +1,48 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      nut;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 2 -1 0 0 0 0];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    inlet
+    {
+        type            calculated;
+        value           uniform 0;
+    }
+
+    freestream
+    {
+        type            calculated;
+        value           uniform 0;
+    }
+
+    wall
+    {
+        type            nutUSpaldingWallFunction;
+        value           uniform 0;
+    }
+
+    processor
+    {
+        type            processor;
+        value           uniform 0;
+    }
+}
+
+// ************************************************************************* //

tutorials/incompressible/simpleFoam/drivaerFastback/0/omega

@@ -0,0 +1,53 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      omega;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+omegaInlet      1.0;
+
+dimensions      [0 0 -1 0 0 0 0];
+
+internalField   uniform $omegaInlet;
+
+boundaryField
+{
+    inlet
+    {
+        type            fixedValue;
+        value           uniform $omegaInlet;
+    }
+
+    freestream
+    {
+        type            inletOutlet;
+        inletValue      uniform $omegaInlet;
+        value           uniform $omegaInlet;
+    }
+
+    wall
+    {
+        type            omegaWallFunction;
+        value           uniform $omegaInlet;
+    }
+
+    processor
+    {
+        type            processor;
+        value           uniform $omegaInlet;
+    }
+
+    #includeEtc "caseDicts/setConstraintTypes"
+}
+
+// ************************************************************************* //

tutorials/incompressible/simpleFoam/drivaerFastback/0/p

@@ -0,0 +1,47 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      p;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 2 -2 0 0 0 0];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    inlet
+    {
+        type            zeroGradient;
+    }
+
+    freestream
+    {
+        type            freestreamPressure;
+        freestreamValue uniform 0;
+        value           uniform 0;
+    }
+
+    wall
+    {
+        type            zeroGradient;
+    }
+
+    processor
+    {
+        type            processor;
+        value           uniform 0;
+    }
+}
+
+// ************************************************************************* //

tutorials/incompressible/simpleFoam/drivaerFastback/Allclean

@@ -0,0 +1,17 @@
+#!/bin/sh
+
+# Run from this directory
+cd "${0%/*}" || exit 1
+
+# Source tutorial clean functions
+. "$WM_PROJECT_DIR/bin/tools/CleanFunctions"
+
+# Delete the following:
+# - time directories
+# - constant/polyMesh directory
+# - postProcessing and VTK directories
+# - log files
+# - field files with a ".orig" backup
+cleanCase
+
+#------------------------------------------------------------------------------

tutorials/incompressible/simpleFoam/drivaerFastback/Allrun

@@ -0,0 +1,23 @@
+#!/bin/sh
+
+# Run from this directory
+cd "${0%/*}" || exit 1
+
+# Source tutorial run functions
+. "$WM_PROJECT_DIR/bin/tools/RunFunctions"
+
+runApplication blockMesh
+
+runApplication decomposePar -copyZero
+
+# echo "Switching to ptscotch for dynamic load balancing with snappyHexMesh"
+# foamDictionary \
+#     -entry method -set ptscotch system/decomposeParDict > /dev/null
+
+runParallel snappyHexMesh -overwrite
+
+runParallel checkMesh
+
+runParallel "$(getApplication)"
+
+#------------------------------------------------------------------------------

tutorials/incompressible/simpleFoam/drivaerFastback/constant/momentumTransport

@@ -0,0 +1,51 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      momentumTransport;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType RAS;
+
+RAS
+{
+    model               kOmegaSST;
+
+    turbulence          on;
+    printCoeffs         on;
+}
+
+LES
+{
+    model               SpalartAllmarasDDES;
+    delta               cubeRootVol;
+
+    turbulence          on;
+    printCoeffs         on;
+
+    cubeRootVolCoeffs
+    {
+        deltaCoeff      1;
+    }
+
+    smoothCoeffs
+    {
+        delta           cubeRootVol;
+        cubeRootVolCoeffs
+        {
+            deltaCoeff      1;
+        }
+        maxDeltaRatio   1.1;
+    }
+}
+
+// ************************************************************************* //

tutorials/incompressible/simpleFoam/drivaerFastback/constant/transportProperties

@@ -0,0 +1,21 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      transportProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+transportModel  Newtonian;
+
+nu              [0 2 -1 0 0 0 0] 1.5e-05;
+
+// ************************************************************************* //

tutorials/incompressible/simpleFoam/drivaerFastback/system/blockMeshDict

@@ -0,0 +1,88 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+xMin   -10;
+xMax    30;
+yMin   -5;
+yMax    5;
+zMin    0;
+zMax    8;
+xCells  80; // 40
+yCells  20; // 10
+zCells  16; //  8
+
+convertToMeters 1;
+
+vertices
+(
+    ($xMin $yMin $zMin)
+    ($xMax $yMin $zMin)
+    ($xMax $yMax $zMin)
+    ($xMin $yMax $zMin)
+
+    ($xMin $yMin $zMax)
+    ($xMax $yMin $zMax)
+    ($xMax $yMax $zMax)
+    ($xMin $yMax $zMax)
+);
+
+blocks
+(
+    hex (0 1 2 3 4 5 6 7) ($xCells $yCells $zCells) simpleGrading (1 1 1)
+);
+
+edges
+(
+);
+
+boundary
+(
+    inlet
+    {
+        type patch;
+        faces
+        (
+            (0 3 7 4)
+        );
+    }
+
+    freestream
+    {
+        type patch;
+        faces
+        (
+            (1 5 6 2)
+            (4 7 6 5)
+            (3 2 6 7)
+            (0 4 5 1)
+        );
+    }
+
+    ground
+    {
+        type wall;
+        faces
+        (
+            (0 1 2 3)
+        );
+    }
+);
+
+mergePatchPairs
+(
+);
+
+// ************************************************************************* //

tutorials/incompressible/simpleFoam/drivaerFastback/system/car

@@ -0,0 +1,30 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+-------------------------------------------------------------------------------
+Description
+    Writes out surface files with interpolated field data in VTK format, e.g.
+    cutting planes, iso-surfaces and patch boundary surfaces.
+
+    This file includes a selection of example surfaces, each of which the user
+    should configure and/or remove.
+
+\*---------------------------------------------------------------------------*/
+
+#includeEtc "caseDicts/postProcessing/visualization/surfaces.cfg"
+
+fields  (p);
+
+surfaces
+(
+    car
+    {
+        $patchSurface;
+        patches  ( ".*(body|Wheels)" );
+    }
+);
+
+// ************************************************************************* //

tutorials/incompressible/simpleFoam/drivaerFastback/system/controlDict

@@ -0,0 +1,60 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application     simpleFoam;
+
+startFrom       latestTime;
+
+startTime       0;
+
+stopAt          endTime;
+
+endTime         1000;
+
+deltaT          1;
+
+writeControl    timeStep;
+
+writeInterval   250;
+
+purgeWrite      0;
+
+writeFormat     binary;
+
+writePrecision   8;
+
+writeCompression off;
+
+timeFormat      general;
+
+timePrecision   6;
+
+runTimeModifiable true;
+
+// adjustTimeStep  yes;
+
+// maxCo           1;
+
+functions
+{
+    #includeFunc forceCoeffsIncompressible
+    #includeFunc time
+    #includeFunc car
+    #includeFunc streamlines
+    #includeFunc slices
+}
+
+// ************************************************************************* //

tutorials/incompressible/simpleFoam/drivaerFastback/system/decomposeParDict.orig

@@ -0,0 +1,29 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      decomposeParDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+numberOfSubdomains  8;
+
+method              scotch;
+//method              hierarchical;
+
+hierarchicalCoeffs
+{
+    n               (4 2 1);
+    delta           0.001;
+    order           xyz;
+}
+
+// ************************************************************************* //

tutorials/incompressible/simpleFoam/drivaerFastback/system/forceCoeffsIncompressible

@@ -0,0 +1,31 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+-------------------------------------------------------------------------------
+Description
+    Calculates lift, drag and moment coefficients by summing forces on
+    specified patches for a case where the solver is incompressible (pressure
+    is kinematic, e.g. m^2/s^2).
+
+\*---------------------------------------------------------------------------*/
+
+#include    "$FOAM_CASE/0/U"
+
+patches     ( ".*(body|Wheels)" );
+
+magUInf     $Uinlet;
+lRef        $wheelBase;
+Aref        2.154;
+
+liftDir     (0 0 1);
+dragDir     (1 0 0);
+
+CofR        (1.391 0 0);
+pitchAxis   (0 1 0);
+
+#includeEtc "caseDicts/postProcessing/forces/forceCoeffsIncompressible.cfg"
+
+// ************************************************************************* //

tutorials/incompressible/simpleFoam/drivaerFastback/system/fvSchemes

@@ -0,0 +1,69 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+    // For transient, replace steadyState, e.g. with Euler
+    default         steadyState;
+}
+
+gradSchemes
+{
+    default         Gauss linear;
+
+    limited         cellLimited Gauss linear 1;
+    grad(U)         $limited;
+    grad(k)         $limited;
+    grad(omega)     $limited;
+}
+
+divSchemes
+{
+    default         none;
+
+    // For transient, remove "bounded"
+    div(phi,U)      bounded Gauss linearUpwind limited;
+
+    // For transient, remove "bounded"
+    turbulence      bounded Gauss limitedLinear 1;
+    div(phi,k)      $turbulence;
+    div(phi,omega)  $turbulence;
+    div(phi,epsilon) $turbulence;
+
+    div((nuEff*dev2(T(grad(U))))) Gauss linear;
+}
+
+laplacianSchemes
+{
+    default         Gauss linear corrected;
+}
+
+interpolationSchemes
+{
+    default         linear;
+}
+
+snGradSchemes
+{
+    default         corrected;
+}
+
+wallDist
+{
+    method meshWave;
+}
+
+// ************************************************************************* //

tutorials/incompressible/simpleFoam/drivaerFastback/system/fvSolution

@@ -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
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+    p
+    {
+        solver          GAMG;
+        smoother        GaussSeidel;
+        tolerance       1e-6;
+        relTol          0.1;
+    }
+
+    pFinal
+    {
+        $p;
+        relTol         0;
+    }
+
+    Phi
+    {
+        $p;
+    }
+
+    "(U|k|omega|epsilon)"
+    {
+        solver          smoothSolver;
+        smoother        symGaussSeidel;
+        tolerance       1e-6;
+        relTol          0.1;
+    }
+
+    "(U|k|omega|epsilon)Final"
+    {
+        $U;
+        relTol          0;
+    }
+}
+
+SIMPLE
+{
+    residualControl
+    {
+        p               1e-4;
+        U               1e-4;
+        "(k|omega|epsilon)" 1e-4;
+    }
+    nNonOrthogonalCorrectors 0;
+    pRefCell        0;
+    pRefValue       0;
+
+}
+
+potentialFlow
+{
+    nNonOrthogonalCorrectors 10;
+}
+
+relaxationFactors
+{
+    fields
+    {
+        p               0.3;
+    }
+    equations
+    {
+        U               0.7;
+        "(k|omega|epsilon)" 0.7;
+    }
+}
+
+// ************************************************************************* //

tutorials/incompressible/simpleFoam/drivaerFastback/system/meshQualityDict

@@ -0,0 +1,22 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      meshQualityDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#includeEtc "caseDicts/mesh/generation/meshQualityDict.cfg"
+
+//- minFaceWeight (0 -> 0.5)
+//minFaceWeight 0.02;
+
+// ************************************************************************* //

tutorials/incompressible/simpleFoam/drivaerFastback/system/slices

@@ -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  |
+-------------------------------------------------------------------------------
+Description
+    Writes out surface files with interpolated field data in VTK format, e.g.
+    cutting planes, iso-surfaces and patch boundary surfaces.
+
+    This file includes a selection of example surfaces, each of which the user
+    should configure and/or remove.
+
+\*---------------------------------------------------------------------------*/
+
+#includeEtc "caseDicts/postProcessing/visualization/surfaces.cfg"
+
+fields  (p U);
+
+surfaces
+(
+    xNormal
+    {
+        $cuttingPlane;
+        pointAndNormalDict
+        {
+            point    (4 0 1);
+            normal   $x;
+        }
+        filtering    full;
+    }
+
+    yNormal
+    {
+        $cuttingPlane;
+        pointAndNormalDict
+        {
+            point    (-5 0.02 1);
+            normal   $y;
+        }
+        filtering    full;
+    }
+);
+
+// ************************************************************************* //

tutorials/incompressible/simpleFoam/drivaerFastback/system/snappyHexMeshDict.orig

@@ -0,0 +1,139 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      snappyHexMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+#includeEtc "caseDicts/mesh/generation/snappyHexMeshDict.cfg"
+
+castellatedMesh on;
+snap            on;
+addLayers       on;
+
+geometry
+{
+    body
+    {
+        type triSurfaceMesh;
+        file "body.obj";
+    }
+
+    frontWheels
+    {
+        type triSurfaceMesh;
+        file "frontWheels.obj";
+    }
+
+    rearWheels
+    {
+        type triSurfaceMesh;
+        file "rearWheels.obj";
+    }
+
+    upstream
+    {
+        type searchableBox;
+        min (-10 -1.5  0);
+        max ( 3   1.5  0.8);
+    }
+
+    underbody
+    {
+        type searchableBox;
+        min (-10 -1.5  0);
+        max ( 3   1.5  0.15);
+    }
+
+    wake
+    {
+        type searchableBox;
+        min ( 3 -1.2  0);
+        max ( 6  1.2 1.4);
+    }
+
+    downstream
+    {
+        type searchableBox;
+        min ( 3 -1.5  0);
+        max (30  1.5 1.8);
+    }
+};
+
+castellatedMeshControls
+{
+    features ();
+
+    refinementSurfaces
+    {
+        body
+        {
+            level (5 5);
+            patchInfo { type wall; }
+        }
+
+        ".*Wheels" // level 5 needed to avoid single cells in treads
+        {
+            level (4 5);
+            patchInfo { type wall; }
+        }
+    }
+
+    refinementRegions
+    {
+        body
+        {
+            mode distance;
+            levels ((0.2 5));
+        }
+
+        "(wake|underbody)"
+        {
+            mode inside;
+            levels ((1E15 4));
+        }
+
+        ".*stream"
+        {
+            mode inside;
+            levels ((1E15 3));
+        }
+    }
+
+    locationInMesh (0 0 3);
+    nCellsBetweenLevels 5;
+}
+
+snapControls {}
+
+addLayersControls
+{
+    layers
+    {
+        body
+        {
+            nSurfaceLayers 2;
+        }
+    }
+
+    relativeSizes       on;
+    expansionRatio      1.2;
+    finalLayerThickness 0.5;
+    minThickness        1e-3;
+    maxThicknessToMedialRatio 0.6;
+}
+
+writeFlags ();
+
+mergeTolerance 1e-6;
+
+// ************************************************************************* //

tutorials/incompressible/simpleFoam/drivaerFastback/system/streamlines

@@ -0,0 +1,28 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+  =========                 |
+  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
+   \\    /   O peration     | Website:  https://openfoam.org
+    \\  /    A nd           | Version:  dev
+     \\/     M anipulation  |
+-------------------------------------------------------------------------------
+Description
+    Writes out files of streamlines with interpolated field data in VTK format.
+
+\*---------------------------------------------------------------------------*/
+
+#includeEtc "caseDicts/postProcessing/visualization/streamlines.cfg"
+
+fields  (U);
+
+direction       both;
+
+seedSampleSet
+{
+    type            sphereRandom;
+    centre          (4 0 0.7);
+    radius          1;
+    nPoints         30;
+    axis x;
+}
+
+// ************************************************************************* //