ENH: Added divergence scheme test case

tutorials/verificationAndValidation/schemes/divergenceExample/0/T

@@ -0,0 +1,51 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  plus                                  |
+|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      T;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 0 0 0 0 0 0];
+
+internalField   uniform 1e-8;
+
+boundaryField
+{
+    top
+    {
+        type            zeroGradient;
+    }
+
+    bottom
+    {
+        type            fixedValue;
+        value           uniform 0;
+    }
+
+    left
+    {
+        type            fixedValue;
+        value           uniform 1;
+    }
+
+    right
+    {
+        type            zeroGradient;
+    }
+
+    frontAndBack
+    {
+        type            empty;
+    }
+}
+
+// ************************************************************************* //

tutorials/verificationAndValidation/schemes/divergenceExample/0/U

@@ -0,0 +1,51 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  plus                                  |
+|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volVectorField;
+    object      U;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 1 -1 0 0 0 0];
+
+internalField   uniform (1 1 0);
+
+boundaryField
+{
+    top
+    {
+        type            zeroGradient;
+    }
+
+    bottom
+    {
+        type            fixedValue;
+        value           $internalField;
+    }
+
+    left
+    {
+        type            fixedValue;
+        value           $internalField;
+    }
+
+    right
+    {
+        type            zeroGradient;
+    }
+
+    frontAndBack
+    {
+        type            empty;
+    }
+}
+
+// ************************************************************************* //

tutorials/verificationAndValidation/schemes/divergenceExample/Allrun

@@ -0,0 +1,21 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # run from this directory
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+
+runApplication blockMesh
+
+cat system/schemesToTest | while read scheme
+do
+    echo "Updating fvSchmes to use $scheme"
+    sed "s/DIVSCHEME/$scheme/g" system/fvSchemes.template > system/fvSchemes
+
+    # Create a sanitised name for the scheme - remove 'special' characters
+    schemeTag=$(sed -e 's# #_#g#' -e 's#(##g' -e 's#)##g' -e 's#\.##g' <<< "$scheme")
+
+    runApplication -s ${schemeTag} scalarTransportFoam
+
+    # Save the line plot
+    mv postProcessing/sample1/100/line1_T.xy line1_T_${schemeTag}.xy
+done

tutorials/verificationAndValidation/schemes/divergenceExample/README

@@ -0,0 +1,17 @@
+Divergence scheme test
+======================
+
+Various divergence schemes are examined on a 2-D structured mesh, where a
+passive scalar is convected at 45deg to the mesh co-ordinate system using a
+uniform flow velocity.  Executing:
+
+./Allrun
+
+will update the system/fvSchemes file to use each scheme listed in the file
+system/schemesToTest and perform the test using the scalarTransportFoam solver.
+A test file for each run is generated that can be used to compare the predicted
+scalar profile against the exact solution.
+
+For more information, see:
+
+https://www.openfoam.com/documentation/cpp-guide/html/guide-schemes-divergence-example.html

tutorials/verificationAndValidation/schemes/divergenceExample/constant/transportProperties

@@ -0,0 +1,21 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  plus                                  |
+|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      transportProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+DT              DT [0 2 -1 0 0] 0;
+
+
+// ************************************************************************* //

tutorials/verificationAndValidation/schemes/divergenceExample/system/blockMeshDict

@@ -0,0 +1,89 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  plus                                  |
+|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+convertToMeters 1;
+
+vertices
+(
+    (0 0 0)
+    (1 0 0)
+    (1 1 0)
+    (0 1 0)
+    (0 0 0.1)
+    (1 0 0.1)
+    (1 1 0.1)
+    (0 1 0.1)
+);
+
+blocks
+(
+    hex (0 1 2 3 4 5 6 7) (50 50 1) simpleGrading (1 1 1)
+);
+
+edges
+(
+);
+
+boundary
+(
+    top
+    {
+        type patch;
+        faces
+        (
+            (3 7 6 2)
+        );
+    }
+    bottom
+    {
+        type patch;
+        faces
+        (
+            (1 5 4 0)
+        );
+    }
+    left
+    {
+        type patch;
+        faces
+        (
+            (0 4 7 3)
+        );
+    }
+    right
+    {
+        type patch;
+        faces
+        (
+            (2 6 5 1)
+        );
+    }
+    frontAndBack
+    {
+        type empty;
+        faces
+        (
+            (0 3 2 1)
+            (4 5 6 7)
+        );
+    }
+);
+
+mergePatchPairs
+(
+);
+
+// ************************************************************************* //

tutorials/verificationAndValidation/schemes/divergenceExample/system/controlDict

@@ -0,0 +1,74 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  plus                                  |
+|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application     scalarTransportFoam;
+
+startFrom       startTime;
+
+startTime       0;
+
+stopAt          endTime;
+
+endTime         100;
+
+deltaT          0.005;
+
+writeControl    timeStep;
+
+writeInterval   100;
+
+purgeWrite      1;
+
+writeFormat     ascii;
+
+writePrecision  6;
+
+writeCompression off;
+
+timeFormat      general;
+
+timePrecision   6;
+
+runTimeModifiable true;
+
+functions
+{
+    sample1
+    {
+        type        sets;
+        functionObjectLibs ("libsampling.so");
+        outputControl onEnd;
+        setFormat   raw;
+        sets
+        (
+            line1
+            {
+                type        uniform;
+                axis        distance;
+
+                // Slightly perturbed so as not to align with face or edge
+                start       (0 1 0.00501);
+                end         (1 0 0.00501);
+                nPoints     200;
+            }
+        );        
+        interpolationScheme cellPoint;
+        fields          (T);
+    }
+}
+
+// ************************************************************************* //

tutorials/verificationAndValidation/schemes/divergenceExample/system/fvSchemes

@@ -0,0 +1,50 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  plus                                  |
+|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+    default         Euler;
+}
+
+gradSchemes
+{
+    default         Gauss linear;
+}
+
+divSchemes
+{
+    default         none;
+    div(phi,T)      Gauss limitedLinear 0.2;
+}
+
+laplacianSchemes
+{
+    default         Gauss linear orthogonal;
+}
+
+interpolationSchemes
+{
+    default         linear;
+}
+
+snGradSchemes
+{
+    default         orthogonal;
+}
+
+
+// ************************************************************************* //

tutorials/verificationAndValidation/schemes/divergenceExample/system/fvSchemes.template

@@ -0,0 +1,50 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  plus                                  |
+|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+    default         Euler;
+}
+
+gradSchemes
+{
+    default         Gauss linear;
+}
+
+divSchemes
+{
+    default         none;
+    div(phi,T)      Gauss DIVSCHEME;
+}
+
+laplacianSchemes
+{
+    default         Gauss linear orthogonal;
+}
+
+interpolationSchemes
+{
+    default         linear;
+}
+
+snGradSchemes
+{
+    default         orthogonal;
+}
+
+
+// ************************************************************************* //

tutorials/verificationAndValidation/schemes/divergenceExample/system/fvSolution

@@ -0,0 +1,37 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| =========                 |                                                 |
+| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
+|  \\    /   O peration     | Version:  plus                                  |
+|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
+|    \\/     M anipulation  |                                                 |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+    T
+    {
+//        solver          smoothSolver;
+//        smoother        symGaussSeidel;
+        solver          PBiCG;
+        preconditioner  DILU;
+        tolerance       1e-10;
+        relTol          0;
+    }
+}
+
+SIMPLE
+{
+    nNonOrthogonalCorrectors 0;
+}
+
+
+// ************************************************************************* //

tutorials/verificationAndValidation/schemes/divergenceExample/system/schemesToTest

@@ -0,0 +1,14 @@
+limitedLinear 0.2
+limitedLinear 1.0
+linear
+linearUpwind grad(U)
+LUST
+midPoint
+Minmod
+MUSCL
+QUICK
+SFCD
+SuperBee
+UMIST
+upwind
+vanLeer