fv::OUForce: New random Ornstein-Uhlenbeck) process force fvModel

Description
    Calculates and applies the random OU (Ornstein-Uhlenbeck) process force to
    the momentum equation for direct numerical simulation of boxes of isotropic
    turbulence.

    The energy spectrum is calculated and written at write-times which is
    particularly useful to test and compare LES SGS models.

Note
    This random OU process force uses a FFT to generate the force field which
    is not currently parallelised.  Also the mesh the FFT is applied to must
    be isotropic and have a power of 2 cells in each direction.

Usage
    Example usage:
    \verbatim
    OUForce
    {
        type    OUForce;

        libs    ("librandomProcesses.so");

        sigma   0.090295;
        alpha   0.81532;
        kUpper  10;
        kLower  7;
    }
    \endverbatim

The tutorials/incompressibleFluid/boxTurb16 tutorial case is an updated version
of the original tutorials/legacy/incompressible/dnsFoam/boxTurb16 case,
demonstrating the use of the OUForce fvModel with the incompressibleFluid solver
module to replicate the behaviour of the legacy dnsFoam solver application.

tutorials/incompressibleFluid/boxTurb16/0/U.orig

@@ -0,0 +1,50 @@
+/*--------------------------------*- 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.orig;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 1 -1 0 0 0 0];
+
+internalField   uniform (0 0 0);
+
+boundaryField
+{
+    patch0_half0
+    {
+        type            cyclic;
+    }
+    patch0_half1
+    {
+        type            cyclic;
+    }
+    patch1_half0
+    {
+        type            cyclic;
+    }
+    patch1_half1
+    {
+        type            cyclic;
+    }
+    patch2_half0
+    {
+        type            cyclic;
+    }
+    patch2_half1
+    {
+        type            cyclic;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/incompressibleFluid/boxTurb16/0/p

@@ -0,0 +1,50 @@
+/*--------------------------------*- 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    "1";
+    object      p;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions      [0 2 -2 0 0 0 0];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    patch0_half0
+    {
+        type            cyclic;
+    }
+    patch1_half0
+    {
+        type            cyclic;
+    }
+    patch2_half0
+    {
+        type            cyclic;
+    }
+    patch2_half1
+    {
+        type            cyclic;
+    }
+    patch1_half1
+    {
+        type            cyclic;
+    }
+    patch0_half1
+    {
+        type            cyclic;
+    }
+}
+
+
+// ************************************************************************* //

tutorials/incompressibleFluid/boxTurb16/Allclean

@@ -0,0 +1,10 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # Run from this directory
+
+# Source tutorial clean functions
+. $WM_PROJECT_DIR/bin/tools/CleanFunctions
+
+cleanCase
+rm -rf 0/enstrophy
+
+#------------------------------------------------------------------------------

tutorials/incompressibleFluid/boxTurb16/Allrun

@@ -0,0 +1,15 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # Run from this directory
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+
+# Get application name
+application=$(getApplication)
+
+runApplication blockMesh
+runApplication boxTurb
+runApplication $application
+runApplication -s enstrophy foamPostProcess -func enstrophy
+
+#------------------------------------------------------------------------------

tutorials/incompressibleFluid/boxTurb16/constant/boxTurbDict

@@ -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
+{
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      boxTurbDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+Ea              10;
+
+k0              5;
+
+
+// ************************************************************************* //

tutorials/incompressibleFluid/boxTurb16/constant/fvModels

@@ -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
+{
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      fvModels;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+OUForce
+{
+    type    OUForce;
+
+    libs    ("librandomProcesses.so");
+
+    sigma   0.090295;
+    alpha   0.81532;
+    kUpper  10;
+    kLower  7;
+}
+
+// ************************************************************************* //

tutorials/incompressibleFluid/boxTurb16/constant/momentumTransport

@@ -0,0 +1,19 @@
+/*--------------------------------*- 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;
+    location    "constant";
+    object      momentumTransport;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType  laminar;
+
+// ************************************************************************* //

tutorials/incompressibleFluid/boxTurb16/constant/physicalProperties

@@ -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
+{
+    format      ascii;
+    class       dictionary;
+    location    "constant";
+    object      physicalProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+viscosityModel  constant;
+
+nu              0.025;
+
+// ************************************************************************* //

tutorials/incompressibleFluid/boxTurb16/system/blockMeshDict

@@ -0,0 +1,94 @@
+/*--------------------------------*- 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 1;
+
+vertices
+(
+    (0 0 0)
+    (1 0 0)
+    (1 1 0)
+    (0 1 0)
+    (0 0 1)
+    (1 0 1)
+    (1 1 1)
+    (0 1 1)
+);
+
+blocks
+(
+    hex (0 1 2 3 4 5 6 7) (16 16 16) simpleGrading (1 1 1)
+);
+
+boundary
+(
+    patch0_half0
+    {
+        type cyclic;
+        neighbourPatch patch0_half1;
+        faces
+        (
+            (0 3 2 1)
+        );
+    }
+    patch0_half1
+    {
+        type cyclic;
+        neighbourPatch patch0_half0;
+        faces
+        (
+            (4 5 6 7)
+        );
+    }
+    patch1_half0
+    {
+        type cyclic;
+        neighbourPatch patch1_half1;
+        faces
+        (
+            (0 4 7 3)
+        );
+    }
+    patch1_half1
+    {
+        type cyclic;
+        neighbourPatch patch1_half0;
+        faces
+        (
+            (2 6 5 1)
+        );
+    }
+    patch2_half0
+    {
+        type cyclic;
+        neighbourPatch patch2_half1;
+        faces
+        (
+            (3 7 6 2)
+        );
+    }
+    patch2_half1
+    {
+        type cyclic;
+        neighbourPatch patch2_half0;
+        faces
+        (
+            (1 5 4 0)
+        );
+    }
+);
+
+
+// ************************************************************************* //

tutorials/incompressibleFluid/boxTurb16/system/controlDict

@@ -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
+{
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application     foamRun;
+
+solver          incompressibleFluid;
+
+startFrom       startTime;
+
+startTime       0;
+
+stopAt          endTime;
+
+endTime         10;
+
+deltaT          0.025;
+
+writeControl    runTime;
+
+writeInterval   0.25;
+
+purgeWrite      0;
+
+writeFormat     ascii;
+
+writePrecision  6;
+
+writeCompression off;
+
+timeFormat      general;
+
+timePrecision   6;
+
+runTimeModifiable true;
+
+graphFormat     raw;
+
+// ************************************************************************* //

tutorials/incompressibleFluid/boxTurb16/system/fvSchemes

@@ -0,0 +1,49 @@
+/*--------------------------------*- 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;
+    location    "system";
+    object      fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+    default         Euler;
+}
+
+gradSchemes
+{
+    default         Gauss linear;
+}
+
+divSchemes
+{
+    default         none;
+    div(phi,U)      Gauss cubic;
+}
+
+laplacianSchemes
+{
+    default         Gauss linear corrected;
+}
+
+interpolationSchemes
+{
+    default         linear;
+}
+
+snGradSchemes
+{
+    default         corrected;
+}
+
+
+// ************************************************************************* //

tutorials/incompressibleFluid/boxTurb16/system/fvSolution

@@ -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       dictionary;
+    location    "system";
+    object      fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+    "p.*"
+    {
+        solver          PCG;
+        preconditioner  DIC;
+        tolerance       1e-06;
+        relTol          0;
+    }
+
+    "U.*"
+    {
+        solver          smoothSolver;
+        smoother        symGaussSeidel;
+        tolerance       1e-05;
+        relTol          0;
+    }
+}
+
+PIMPLE
+{
+    nCorrectors     2;
+    nNonOrthogonalCorrectors 0;
+    pRefCell        0;
+    pRefValue       0;
+}
+
+
+// ************************************************************************* //

tutorials/legacy/incompressible/dnsFoam/boxTurb16/constant/momentumTransport

@@ -14,13 +14,9 @@ FoamFile
 }
 // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
-UOsigma         0.090295;
-
-UOalpha         0.81532;
-
-UOKupper        10;
-
-UOKlower        7;
-
+sigma   0.090295;
+alpha   0.81532;
+kUpper  10;
+kLower  7;
 
 // ************************************************************************* //