Skip to content
GitLab
Commit 8c8a3a16 authored by Henry Weller's avatar Henry Weller
Browse files

tutorials/incompressible/simpleFoam/rotorDisk: Tutorial for the rotorDiskSource functionObject 

Provided by Richard Jones
parent c77e033a
Expand all Hide whitespace changes
Inline Side-by-side
src/fvOptions/sources/derived/rotorDiskSource/rotorDiskSource.H
View file @ 8c8a3a16
......@@ -25,10 +25,10 @@ Class
Foam::fv::rotorDiskSource
Description
Cell based momemtum source
Rotor disk source
Source approximates the mean effects of rotor forces on a cylindrical
region within the domain
Cell based momemtum source which approximates the mean effects of
rotor forces on a cylindrical region within the domain.
\heading Source usage
......
tutorials/incompressible/simpleFoam/rotorDisk/0/U 0 → 100644
View file @ 8c8a3a16
/*--------------------------------*- 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;
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Uinlet (0 1 0);
dimensions [0 1 -1 0 0 0 0];
internalField uniform $Uinlet;
boundaryField
{
inlet
{
type fixedValue;
value uniform $Uinlet;
}
outlet
{
type pressureInletOutletVelocity;
value uniform $Uinlet;
}
"slip.*"
{
type slip;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //
tutorials/incompressible/simpleFoam/rotorDisk/0/k 0 → 100644
View file @ 8c8a3a16
/*--------------------------------*- 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;
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
kInlet 0.02;
dimensions [0 2 -2 0 0 0 0];
internalField uniform $kInlet;
boundaryField
{
inlet
{
type fixedValue;
value uniform $kInlet;
}
outlet
{
type inletOutlet;
inletValue uniform $kInlet;
value uniform $kInlet;
}
"slip.*"
{
type slip;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //
tutorials/incompressible/simpleFoam/rotorDisk/0/nut 0 → 100644
View file @ 8c8a3a16
/*--------------------------------*- 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;
object nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -1 0 0 0 0];
internalField uniform 0;
boundaryField
{
inlet
{
type calculated;
value uniform 0;
}
outlet
{
type calculated;
value uniform 0;
}
"slip.*"
{
type slip;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //
tutorials/incompressible/simpleFoam/rotorDisk/0/omega 0 → 100644
View file @ 8c8a3a16
/*--------------------------------*- 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;
object omega;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
omegaInlet 10.0;
dimensions [0 0 -1 0 0 0 0];
internalField uniform $omegaInlet;
boundaryField
{
inlet
{
type fixedValue;
value uniform $omegaInlet;
}
outlet
{
type inletOutlet;
inletValue uniform $omegaInlet;
value uniform $omegaInlet;
}
"slip.*"
{
type slip;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //
tutorials/incompressible/simpleFoam/rotorDisk/0/p 0 → 100644
View file @ 8c8a3a16
/*--------------------------------*- 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;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -2 0 0 0 0];
internalField uniform 0;
boundaryField
{
inlet
{
type zeroGradient;
}
outlet
{
type fixedValue;
value uniform 0;
}
"slip.*"
{
type slip;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //
tutorials/incompressible/simpleFoam/rotorDisk/Allclean 0 → 100755
View file @ 8c8a3a16
#!/bin/sh
# Source tutorial clean functions
. $WM_PROJECT_DIR/bin/tools/CleanFunctions
# remove surface and features
\rm -rf constant/extendedFeatureEdgeMesh > /dev/null 2>&1
\rm -f constant/triSurface/rotatingZone.eMesh > /dev/null 2>&1
\rm -f constant/triSurface/fixed.eMesh > /dev/null 2>&1
\rm -f 0/pointLevel > /dev/null 2>&1
\rm -f 0/cellLevel > /dev/null 2>&1
cleanCase
tutorials/incompressible/simpleFoam/rotorDisk/Allrun 0 → 100755
View file @ 8c8a3a16
#!/bin/sh
cd ${0%/*} || exit 1 # Run from this directory
# Source tutorial run functions
. $WM_PROJECT_DIR/bin/tools/RunFunctions
# Meshing
runApplication blockMesh
runApplication surfaceFeatureExtract
runApplication snappyHexMesh -overwrite
runApplication createPatch -overwrite
runApplication $(getApplication)
# ----------------------------------------------------------------- end-of-file
tutorials/incompressible/simpleFoam/rotorDisk/constant/polyMesh/boundary 0 → 100644
View file @ 8c8a3a16
/*--------------------------------*- 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 polyBoundaryMesh;
location "constant/polyMesh";
object boundary;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
3
(
slipWall
{
type slip;
inGroups 1(slip);
nFaces 11616;
startFace 215580;
inGroups 1 ( slip );
}
outlet
{
type patch;
nFaces 1788;
startFace 227196;
}
inlet
{
type patch;
nFaces 1788;
startFace 228984;
}
)
// ************************************************************************* //
tutorials/incompressible/simpleFoam/rotorDisk/constant/transportProperties 0 → 100644
View file @ 8c8a3a16
/*--------------------------------*- 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 transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
transportModel Newtonian;
nu nu [ 0 2 -1 0 0 0 0 ] 1.5e-05;
// ************************************************************************* //
tutorials/incompressible/simpleFoam/rotorDisk/constant/turbulenceProperties 0 → 100644
View file @ 8c8a3a16
/*--------------------------------*- 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 turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
simulationType RAS;
RAS
{
RASModel kOmegaSST;
turbulence on;
printCoeffs on;
}
// ************************************************************************* //
tutorials/incompressible/simpleFoam/rotorDisk/system/blockMeshDict 0 → 100644
View file @ 8c8a3a16
/*--------------------------------*- 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 blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
backgroundMesh
{
xMin -1.26;
xMax 1.26;
yMin -2.01;
yMax 2.01;
zMin -1.26;
zMax 1.26;
xCells 12;
yCells 22;
zCells 12;
}
convertToMeters 1;
vertices
(
($:backgroundMesh.xMin $:backgroundMesh.yMin $:backgroundMesh.zMin)
($:backgroundMesh.xMax $:backgroundMesh.yMin $:backgroundMesh.zMin)
($:backgroundMesh.xMax $:backgroundMesh.yMax $:backgroundMesh.zMin)
($:backgroundMesh.xMin $:backgroundMesh.yMax $:backgroundMesh.zMin)
($:backgroundMesh.xMin $:backgroundMesh.yMin $:backgroundMesh.zMax)
($:backgroundMesh.xMax $:backgroundMesh.yMin $:backgroundMesh.zMax)
($:backgroundMesh.xMax $:backgroundMesh.yMax $:backgroundMesh.zMax)
($:backgroundMesh.xMin $:backgroundMesh.yMax $:backgroundMesh.zMax)
);
blocks
(
hex (0 1 2 3 4 5 6 7)
(
$:backgroundMesh.xCells
$:backgroundMesh.yCells
$:backgroundMesh.zCells
)
simpleGrading (1 1 1)
);
edges
(
);
boundary
(
);
mergePatchPairs
(
);
// ************************************************************************* //
tutorials/incompressible/simpleFoam/rotorDisk/system/controlDict 0 → 100644
View file @ 8c8a3a16
/*--------------------------------*- 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 controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application simpleFoam;
startFrom startTime;
startTime 0;
stopAt endTime;
endTime 1000;
deltaT 1;
writeControl timeStep;
writeInterval 50;
purgeWrite 0;
writeFormat ascii;
writePrecision 8;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable true;
// ************************************************************************* //
tutorials/incompressible/simpleFoam/rotorDisk/system/createPatchDict 0 → 100644
View file @ 8c8a3a16
/*--------------------------------*- 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 createPatchDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
// Do a synchronisation of coupled points after creation of any patches.
// Note: this does not work with points that are on multiple coupled patches
// with transformations (i.e. cyclics).
pointSync false;
// Patches to create. An empty patch list just removes patches with zero
// faces from $FOAM_CASE/constant/polyMesh/boundary.
patches
(
);
// ************************************************************************* //
tutorials/incompressible/simpleFoam/rotorDisk/system/fvOptions 0 → 100644
View file @ 8c8a3a16
/*--------------------------------*- 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 fvOptions;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
disk
{
type rotorDisk;
active on;
rotorDiskCoeffs
{
selectionMode cellZone;
cellZone rotatingZone;
fieldNames (U); // Names of fields on which to apply source
nBlades 3; // Number of blades
tipEffect 0.96; // Normalised radius above which lift = 0
inletFlowType local; // Inlet flow type specification
inletVelocity (0 1 0);
geometryMode specified;
origin (0 0 0);
axis (0 1 0);
refDirection (0 0 1); // Reference direction
// - used as reference for psi angle
rpm 1000;
//pointAbove (0 0 0.25);
trimModel fixedTrim; // fixed || targetForce
rhoRef 1000;
rhoInf 1;
fixedTrimCoeffs
{
theta0 0;
theta1c 0;
theta1s 0;
}
flapCoeffs
{
beta0 0; // Coning angle [deg]
beta1c 0; // Lateral flapping coeff (cos coeff)
beta2s 0; // Longitudinal flapping coeff (sin coeff)
}
blade
{
data
(
(profile1 (0.1 -6 0.1))
(profile1 (0.25 -6 0.1))
);
}
profiles
{
profile1
{
type lookup;
data
(
(-90 0.21 1.45)
(-18 0.21 1.45)
(-16 0.165 1.3)
(-14 0.125 1.1)
(-12 0.092 0.95)
(-10 0.07 0.8)
(-8 0.05 0.64)
(-6 0.04 0.5)
(-4 0.028 0.32)
(-2 0.022 0.18)
(0 0.02 0)
(2 0.022 0.18)
(4 0.028 0.32)
(6 0.04 0.5)
(8 0.05 0.64)
(10 0.07 0.8)
(12 0.092 0.95)
(14 0.125 1.1)