songtianlun/openfoam
1
0
Fork 0
Code Issues Pull Requests Actions Packages Projects Releases Wiki Activity

DTCHull: new interDyMFoam tutorial

Browse Source
This commit is contained in:
Henry 2014-02-01 17:14:35 +00:00
parent bf0a90d570
commit 34bc9cadb0
31 changed files with 1782 additions and 0 deletions
Show Stats Download Patch File Download Diff File Expand all files Collapse all files

58
tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/U Normal file
View File

@ -0,0 +1,58 @@
/*--------------------------------*- 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;
location "0";
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Umean 1.668;
mUmean -1.668;
dimensions [0 1 -1 0 0 0 0];
internalField uniform ($mUmean 0 0);
boundaryField
{
//- Set patchGroups for constraint patches
#include "${WM_PROJECT_DIR}/etc/caseDicts/setConstraintTypes"
inlet
{
type fixedValue;
value $internalField;
}
outlet
{
type outletPhaseMeanVelocity;
alpha alpha.water;
Umean $Umean;
value $internalField;
}
atmosphere
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
}
hull
{
type movingWallVelocity;
value uniform (0 0 0);
}
}
// ************************************************************************* //

54
tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/alpha.water Normal file
View File

@ -0,0 +1,54 @@
/*--------------------------------*- 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;
location "0";
object alpha;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 0 0 0 0];
internalField uniform 0;
boundaryField
{
//- Set patchGroups for constraint patches
#include "${WM_PROJECT_DIR}/etc/caseDicts/setConstraintTypes"
inlet
{
type fixedValue;
value $internalField;
}
outlet
{
type variableHeightFlowRate;
lowerBound 0;
upperBound 1;
value $internalField;
}
atmosphere
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
hull
{
type zeroGradient;
}
}
// ************************************************************************* //

54
tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/k Normal file
View File

@ -0,0 +1,54 @@
/*--------------------------------*- 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;
location "0";
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -2 0 0 0 0];
internalField uniform 0.00015;
boundaryField
{
//- Set patchGroups for constraint patches
#include "${WM_PROJECT_DIR}/etc/caseDicts/setConstraintTypes"
inlet
{
type fixedValue;
value $internalField;
}
outlet
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
atmosphere
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
hull
{
type kqRWallFunction;
value $internalField;
}
}
// ************************************************************************* //

53
tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/nut Normal file
View File

@ -0,0 +1,53 @@
/*--------------------------------*- 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;
location "0";
object nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -1 0 0 0 0];
internalField uniform 5e-07;
boundaryField
{
//- Set patchGroups for constraint patches
#include "${WM_PROJECT_DIR}/etc/caseDicts/setConstraintTypes"
inlet
{
type fixedValue;
value $internalField;
}
outlet
{
type zeroGradient;
}
atmosphere
{
type zeroGradient;
}
hull
{
type nutkRoughWallFunction;
Ks uniform 100e-6;
Cs uniform 0.5;
value $internalField;
}
}
// ************************************************************************* //

56
tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/omega Normal file
View File

@ -0,0 +1,56 @@
/*--------------------------------*- 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;
location "0";
object omega;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 -1 0 0 0 0];
internalField uniform 2;
boundaryField
{
//- Set patchGroups for constraint patches
#include "${WM_PROJECT_DIR}/etc/caseDicts/setConstraintTypes"
inlet
{
type fixedValue;
value $internalField;
}
outlet
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
atmosphere
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
hull
{
type omegaWallFunction;
value $internalField;
}
}
// ************************************************************************* //

57
tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/p_rgh Normal file
View File

@ -0,0 +1,57 @@
/*--------------------------------*- 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;
location "0";
object p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -2 0 0 0 0];
internalField uniform 0;
boundaryField
{
//- Set patchGroups for constraint patches
#include "${WM_PROJECT_DIR}/etc/caseDicts/setConstraintTypes"
inlet
{
type fixedFluxPressure;
value $internalField;
}
outlet
{
type zeroGradient;
}
atmosphere
{
type totalPressure;
p0 uniform 0;
U U;
phi phi;
rho rho;
psi none;
gamma 1;
value $internalField;
}
hull
{
type fixedFluxPressure;
value $internalField;
}
}
// ************************************************************************* //

52
tutorials/multiphase/interDyMFoam/ras/DTCHull/0.org/pointDisplacement Normal file
View File

@ -0,0 +1,52 @@
/*--------------------------------*- 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 pointVectorField;
location "0";
object pointDisplacement;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 0 0 0 0 0];
internalField uniform (0 0 0);
boundaryField
{
//- Set patchGroups for constraint patches
#include "${WM_PROJECT_DIR}/etc/caseDicts/setConstraintTypes"
inlet
{
type fixedValue;
value uniform (0 0 0);
}
outlet
{
type fixedValue;
value uniform (0 0 0);
}
atmosphere
{
type fixedValue;
value uniform (0 0 0);
}
hull
{
type calculated;
}
}
// ************************************************************************* //

17
tutorials/multiphase/interDyMFoam/ras/DTCHull/Allclean Executable file
View File

@ -0,0 +1,17 @@
#!/bin/sh
cd ${0%/*} || exit 1 # run from this directory
# Source tutorial clean functions
. $WM_PROJECT_DIR/bin/tools/CleanFunctions
# remove surface
\rm -f constant/triSurface/DTC-scaled.stl.gz > /dev/null 2>&1
\rm -rf constant/extendedFeatureEdgeMesh > /dev/null 2>&1
\rm -f constant/triSurface/DTC-scaled.eMesh > /dev/null 2>&1
cleanCase
\rm constant/polyMesh/boundary > /dev/null 2>&1
\rm -rf 0 > /dev/null 2>&1
\rm system/topoSetDict > /dev/null 2>&1
# ----------------------------------------------------------------- end-of-file

48
tutorials/multiphase/interDyMFoam/ras/DTCHull/Allrun Executable file
View File

@ -0,0 +1,48 @@
#!/bin/sh
cd ${0%/*} || exit 1 # run from this directory
# Source tutorial run functions
. $WM_PROJECT_DIR/bin/tools/RunFunctions
runRefineMesh ()
{
echo "Running refineMesh on $PWD"
refineMesh -dict system/refineMeshDict -overwrite > log.refineMesh 2>&1
}
# copy DTC hull surface from resources folder
cp $FOAM_TUTORIALS/resources/geometry/DTC-scaled.stl.gz constant/triSurface/
runApplication surfaceFeatureExtract
runApplication blockMesh
i=1
if [ -f log.topoSet.6 ] ; then
i=7
fi
while [ "$i" -lt 7 ] ; do
cp system/topoSetDict.${i} system/topoSetDict
runApplication topoSet
runRefineMesh
mv log.topoSet log.topoSet.$i
mv log.refineMesh log.refineMesh.$i
i=$(expr $i + 1)
done
runApplication snappyHexMesh -overwrite
\rm -rf 0
\cp -r 0.org 0
runApplication setFields
runApplication decomposePar
runParallel renumberMesh 8 -overwrite
runParallel $(getApplication) 8
runApplication reconstructPar
# ----------------------------------------------------------------- end-of-file

25
tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/RASProperties Normal file
View File

@ -0,0 +1,25 @@
/*--------------------------------*- 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;
location "constant";
object RASProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
RASModel kOmegaSST;
turbulence on;
printCoeffs on;
// ************************************************************************* //

67
tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/dynamicMeshDict Normal file
View File

@ -0,0 +1,67 @@
/*--------------------------------*- 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 dynamicMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dynamicFvMesh dynamicMotionSolverFvMesh;
motionSolverLibs ("libsixDoFRigidBodyMotion.so");
solver sixDoFRigidBodyMotion;
sixDoFRigidBodyMotionCoeffs
{
patches (hull);
innerDistance 0.3;
outerDistance 1;
centreOfMass (2.929541 0 0.2);
mass 412.73;
momentOfInertia (40 921 921);
rhoInf 1;
report on;
accelerationRelaxation 0.3;
value uniform (0 0 0);
constraints
{
zAxis
{
sixDoFRigidBodyMotionConstraint line;
direction (0 0 1);
}
yPlane
{
sixDoFRigidBodyMotionConstraint axis;
axis (0 1 0);
}
}
restraints
{
translationDamper
{
sixDoFRigidBodyMotionRestraint linearDamper;
coeff 8596;
}
rotationDamper
{
sixDoFRigidBodyMotionRestraint sphericalAngularDamper;
coeff 11586;
}
}
}
// ************************************************************************* //

21
tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/g Normal file
View File

@ -0,0 +1,21 @@
/*--------------------------------*- 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 uniformDimensionedVectorField;
location "constant";
object g;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -2 0 0 0 0];
value (0 0 -9.81);
// ************************************************************************* //

147
tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/polyMesh/blockMeshDict Normal file
View File

@ -0,0 +1,147 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 1;
vertices
(
(-26 -19 -16)
(16 -19 -16)
(16 0 -16)
(-26 0 -16)
(-26 -19 -1)
(16 -19 -1)
(16 0 -1)
(-26 0 -1)
(-26 -19 0.185)
(16 -19 0.185)
(16 0 0.185)
(-26 0 0.185)
(-26 -19 0.244)
(16 -19 0.244)
(16 0 0.244)
(-26 0 0.244)
(-26 -19 0.3)
(16 -19 0.3)
(16 0 0.3)
(-26 0 0.3)
(-26 -19 1.6)
(16 -19 1.6)
(16 0 1.6)
(-26 0 1.6)
(-26 -19 4)
(16 -19 4)
(16 0 4)
(-26 0 4)
);
blocks
(
hex (0 1 2 3 4 5 6 7) (42 19 50) simpleGrading (1 1 0.05)
hex (4 5 6 7 8 9 10 11) (42 19 50) simpleGrading (1 1 1)
hex (8 9 10 11 12 13 14 15) (42 19 4) simpleGrading (1 1 1)
hex (12 13 14 15 16 17 18 19) (42 19 4) simpleGrading (1 1 1)
hex (16 17 18 19 20 21 22 23) (42 19 40) simpleGrading (1 1 1)
hex (20 21 22 23 24 25 26 27) (42 19 20) simpleGrading (1 1 5)
);
edges
(
);
boundary
(
atmosphere
{
type patch;
faces
(
(24 25 26 27)
);
}
inlet
{
type patch;
faces
(
(1 2 6 5)
(5 6 10 9)
(9 10 14 13)
(13 14 18 17)
(17 18 22 21)
(21 22 26 25)
);
}
outlet
{
type patch;
faces
(
(0 4 7 3)
(4 8 11 7)
(8 12 15 11)
(12 16 19 15)
(16 20 23 19)
(20 24 27 23)
);
}
bottom
{
type symmetryPlane;
faces
(
(0 3 2 1)
);
}
side
{
type symmetryPlane;
faces
(
(0 1 5 4)
(4 5 9 8)
(8 9 13 12)
(12 13 17 16)
(16 17 21 20)
(20 21 25 24)
);
}
midPlane
{
type symmetryPlane;
faces
(
(3 7 6 2)
(7 11 10 6)
(11 15 14 10)
(15 19 18 14)
(19 23 22 18)
(23 27 26 22)
);
}
);
mergePatchPairs
(
);
// ************************************************************************* //

36
tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/transportProperties Normal file
View File

@ -0,0 +1,36 @@
/*--------------------------------*- 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;
location "constant";
object transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
phases (water air);
water
{
transportModel Newtonian;
nu nu [ 0 2 -1 0 0 0 0 ] 1.09e-06;
rho rho [ 1 -3 0 0 0 0 0 ] 998.8;
}
air
{
transportModel Newtonian;
nu nu [ 0 2 -1 0 0 0 0 ] 1.48e-05;
rho rho [ 1 -3 0 0 0 0 0 ] 1;
}
sigma sigma [ 1 0 -2 0 0 0 0 ] 0;
// ************************************************************************* //

4
tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/triSurface/README Normal file
View File

@ -0,0 +1,4 @@
Folder to house tri-surfaces
The Allrun script copies the surface from the $FOAM_TUTORIALS/resources/geometry
folder

21
tutorials/multiphase/interDyMFoam/ras/DTCHull/constant/turbulenceProperties Normal file
View File

@ -0,0 +1,21 @@
/*--------------------------------*- 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;
location "constant";
object turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
simulationType RASModel;
// ************************************************************************* //

72
tutorials/multiphase/interDyMFoam/ras/DTCHull/system/controlDict Normal file
View File

@ -0,0 +1,72 @@
/*--------------------------------*- 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;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application interDyMFoam;
startFrom startTime;
startTime 0;
stopAt endTime;
endTime 50;
deltaT 0.0001;
writeControl adjustableRunTime;
writeInterval 5;
purgeWrite 0;
writeFormat binary;
writePrecision 6;
writeCompression uncompressed;
timeFormat general;
timePrecision 6;
runTimeModifiable yes;
adjustTimeStep yes;
maxCo 25;
maxAlphaCo 15;
maxDeltaT 0.01;
functions
{
forces
{
type forces;
functionObjectLibs ( "libforces.so" );
patches (hull);
rhoInf 998.8;
rhoName rho;
UName U;
log on;
outputControl timeStep;
outputInterval 1;
CofR (2.929541 0 0.2);
}
}
// ************************************************************************* //

58
tutorials/multiphase/interDyMFoam/ras/DTCHull/system/decomposeParDict Normal file
View File

@ -0,0 +1,58 @@
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.4 |
| \\ / A nd | Web: http://www.openfoam.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
root "";
case "";
instance "";
local "";
class dictionary;
object decomposeParDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
numberOfSubdomains 8;
method scotch;
simpleCoeffs
{
n (2 1 1);
delta 0.001;
}
hierarchicalCoeffs
{
n (1 1 1);
delta 0.001;
order xyz;
}
metisCoeffs
{
}
manualCoeffs
{
dataFile "";
}
distributed no;
roots
(
);
// ************************************************************************* //

63
tutorials/multiphase/interDyMFoam/ras/DTCHull/system/fvSchemes Normal file
View File

@ -0,0 +1,63 @@
/*--------------------------------*- 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;
location "system";
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
default Euler;
}
gradSchemes
{
default Gauss linear;
limitedGrad cellLimited Gauss linear 1;
}
divSchemes
{
div(rhoPhi,U) Gauss linearUpwind grad(U);
div(phi,alpha) Gauss vanLeer;
div(phirb,alpha) Gauss linear;
div(phi,k) Gauss linearUpwind limitedGrad;
div(phi,omega) Gauss linearUpwind limitedGrad;
div((muEff*dev(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default corrected;
}
fluxRequired
{
default no;
p_rgh;
pcorr;
alpha.water;
}
// ************************************************************************* //

117
tutorials/multiphase/interDyMFoam/ras/DTCHull/system/fvSolution Normal file
View File

@ -0,0 +1,117 @@
/*--------------------------------*- 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;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
"alpha.water.*"
{
nAlphaCorr 3;
nAlphaSubCycles 1;
cAlpha 1;
icAlpha 0;
alphaOuterCorrectors yes;
MULESCorr yes;
nLimiterIter 10;
alphaApplyPrevCorr yes;
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-10;
relTol 0;
minIter 1;
}
"pcorr.*"
{
solver GAMG;
smoother DIC;
agglomerator faceAreaPair;
mergeLevels 1;
nCellsInCoarsestLevel 10;
cacheAgglomeration true;
tolerance 0.1;
relTol 0;
};
p_rgh
{
solver GAMG;
smoother DIC;
agglomerator faceAreaPair;
mergeLevels 1;
nCellsInCoarsestLevel 10;
cacheAgglomeration true;
tolerance 5e-8;
relTol 0.001;
};
p_rghFinal
{
$p_rgh;
relTol 0;
}
"(U|k|omega).*"
{
solver smoothSolver;
smoother symGaussSeidel;
nSweeps 1;
tolerance 1e-7;
relTol 0;
minIter 1;
};
}
PIMPLE
{
momentumPredictor no;
nOuterCorrectors 1;
nCorrectors 3;
nNonOrthogonalCorrectors 0;
correctPhi yes;
moveMeshOuterCorrectors yes;
turbOnFinalIterOnly yes;
}
relaxationFactors
{
fields
{
}
equations
{
".*" 1;
}
}
cache
{
grad(U);
}
// ************************************************************************* //

86
tutorials/multiphase/interDyMFoam/ras/DTCHull/system/meshQualityDict Normal file
View File

@ -0,0 +1,86 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.x |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object meshQualityDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
//- Maximum non-orthogonality allowed. Set to 180 to disable.
maxNonOrtho 70;
//- Max skewness allowed. Set to <0 to disable.
maxBoundarySkewness 20;
maxInternalSkewness 4;
//- Max concaveness allowed. Is angle (in degrees) below which concavity
// is allowed. 0 is straight face, <0 would be convex face.
// Set to 180 to disable.
maxConcave 80;
//- Minimum pyramid volume. Is absolute volume of cell pyramid.
// Set to a sensible fraction of the smallest cell volume expected.
// Set to very negative number (e.g. -1E30) to disable.
minVol 1e-13;
//- Minimum quality of the tet formed by the face-centre
// and variable base point minimum decomposition triangles and
// the cell centre. Set to very negative number (e.g. -1E30) to
// disable.
// <0 = inside out tet,
// 0 = flat tet
// 1 = regular tet
minTetQuality 1e-30;
//- Minimum face area. Set to <0 to disable.
minArea -1;
//- Minimum face twist. Set to <-1 to disable. dot product of face normal
//- and face centre triangles normal
minTwist 0.05;
//- minimum normalised cell determinant
//- 1 = hex, <= 0 = folded or flattened illegal cell
minDeterminant 0.001;
//- minFaceWeight (0 -> 0.5)
minFaceWeight 0.05;
//- minVolRatio (0 -> 1)
minVolRatio 0.01;
//must be >0 for Fluent compatibility
minTriangleTwist -1;
//- if >0 : preserve single cells with all points on the surface if the
// resulting volume after snapping (by approximation) is larger than
// minVolCollapseRatio times old volume (i.e. not collapsed to flat cell).
// If <0 : delete always.
//minVolCollapseRatio 0.5;
// Advanced
//- Number of error distribution iterations
nSmoothScale 4;
//- amount to scale back displacement at error points
errorReduction 0.75;
// Optional : some meshing phases allow usage of relaxed rules.
// See e.g. addLayersControls::nRelaxedIter.
relaxed
{
//- Maximum non-orthogonality allowed. Set to 180 to disable.
maxNonOrtho 75;
}

43
tutorials/multiphase/interDyMFoam/ras/DTCHull/system/refineMeshDict Normal file
View File

@ -0,0 +1,43 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object refineMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
set c0;
coordinateSystem global;
globalCoeffs
{
tan1 ( 1 0 0 );
tan2 ( 0 1 0 );
}
patchLocalCoeffs
{
patch outside;
tan1 ( 1 0 0 );
}
directions ( tan1 tan2 );
useHexTopology no;
geometricCut yes;
writeMesh no;
// ************************************************************************* //

49
tutorials/multiphase/interDyMFoam/ras/DTCHull/system/setFieldsDict Normal file
View File

@ -0,0 +1,49 @@
/*--------------------------------*- 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;
location "system";
object setFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
defaultFieldValues
(
volScalarFieldValue alpha.water 0
);
regions
(
// Set cell values
// (does zerogradient on boundaries)
boxToCell
{
box (-999 -999 -999) (999 999 0.244);
fieldValues
(
volScalarFieldValue alpha.water 1
);
}
// Set patch values (using ==)
boxToFace
{
box (-999 -999 -999) (999 999 0.244);
fieldValues
(
volScalarFieldValue alpha.water 1
);
}
);
// ************************************************************************* //

284
tutorials/multiphase/interDyMFoam/ras/DTCHull/system/snappyHexMeshDict Normal file
View File

@ -0,0 +1,284 @@
/*--------------------------------*- 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 snappyHexMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
// Which of the steps to run
castellatedMesh true;
snap true;
addLayers true;
// Geometry. Definition of all surfaces. All surfaces are of class
// searchableSurface.
// Surfaces are used
// - to specify refinement for any mesh cell intersecting it
// - to specify refinement for any mesh cell inside/outside/near
// - to 'snap' the mesh boundary to the surface
geometry
{
DTC-scaled.stl
{
type triSurfaceMesh;
name hull;
patchInfo
{
type wall;
}
}
};
// Settings for the castellatedMesh generation.
castellatedMeshControls
{
// Refinement parameters
// ~~~~~~~~~~~~~~~~~~~~~
// If local number of cells is >= maxLocalCells on any processor
// switches from from refinement followed by balancing
// (current method) to (weighted) balancing before refinement.
maxLocalCells 100000;
// Overall cell limit (approximately). Refinement will stop immediately
// upon reaching this number so a refinement level might not complete.
// Note that this is the number of cells before removing the part which
// is not 'visible' from the keepPoint. The final number of cells might
// actually be a lot less.
maxGlobalCells 2000000;
// The surface refinement loop might spend lots of iterations refining just a
// few cells. This setting will cause refinement to stop if <= minimumRefine
// are selected for refinement. Note: it will at least do one iteration
// (unless the number of cells to refine is 0)
minRefinementCells 0;
// Number of buffer layers between different levels.
// 1 means normal 2:1 refinement restriction, larger means slower
// refinement.
nCellsBetweenLevels 3;
// Explicit feature edge refinement
// ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
// Specifies a level for any cell intersected by its edges.
// This is a featureEdgeMesh, read from constant/triSurface for now.
features
(
{
file "DTC-scaled.eMesh";
level 0;
}
);
// Surface based refinement
// ~~~~~~~~~~~~~~~~~~~~~~~~
// Specifies two levels for every surface. The first is the minimum level,
// every cell intersecting a surface gets refined up to the minimum level.
// The second level is the maximum level. Cells that 'see' multiple
// intersections where the intersections make an
// angle > resolveFeatureAngle get refined up to the maximum level.
refinementSurfaces
{
hull
{
// Surface-wise min and max refinement level
level (0 0);
}
}
resolveFeatureAngle 45;
// Region-wise refinement
// ~~~~~~~~~~~~~~~~~~~~~~
// Specifies refinement level for cells in relation to a surface. One of
// three modes
// - distance. 'levels' specifies per distance to the surface the
// wanted refinement level. The distances need to be specified in
// descending order.
// - inside. 'levels' is only one entry and only the level is used. All
// cells inside the surface get refined up to the level. The surface
// needs to be closed for this to be possible.
// - outside. Same but cells outside.
refinementRegions
{
}
// Mesh selection
// ~~~~~~~~~~~~~~
// After refinement patches get added for all refinementSurfaces and
// all cells intersecting the surfaces get put into these patches. The
// section reachable from the locationInMesh is kept.
// NOTE: This point should never be on a face, always inside a cell, even
// after refinement.
locationInMesh (-0.7 0 0);
// Whether any faceZones (as specified in the refinementSurfaces)
// are only on the boundary of corresponding cellZones or also allow
// free-standing zone faces. Not used if there are no faceZones.
allowFreeStandingZoneFaces true;
}
// Settings for the snapping.
snapControls
{
//- Number of patch smoothing iterations before finding correspondence
// to surface
nSmoothPatch 3;
//- Relative distance for points to be attracted by surface feature point
// or edge. True distance is this factor times local
// maximum edge length.
// tolerance 4.0;
tolerance 1.0;
//- Number of mesh displacement relaxation iterations.
nSolveIter 100;
//- Maximum number of snapping relaxation iterations. Should stop
// before upon reaching a correct mesh.
nRelaxIter 5;
nFeatureSnapIter 10;
}
// Settings for the layer addition.
addLayersControls
{
// Are the thickness parameters below relative to the undistorted
// size of the refined cell outside layer (true) or absolute sizes (false).
relativeSizes true;
// Per final patch (so not geometry!) the layer information
layers
{
hull
{
nSurfaceLayers 3;
}
}
// Expansion factor for layer mesh
expansionRatio 1.5;
// Wanted thickness of final added cell layer. If multiple layers
// is the thickness of the layer furthest away from the wall.
// See relativeSizes parameter.
finalLayerThickness 0.7;
// Minimum thickness of cell layer. If for any reason layer
// cannot be above minThickness do not add layer.
// See relativeSizes parameter.
minThickness 0.25;
// If points get not extruded do nGrow layers of connected faces that are
// also not grown. This helps convergence of the layer addition process
// close to features.
// Note: changed(corrected) w.r.t 17x! (didn't do anything in 17x)
nGrow 0;
// Advanced settings
// When not to extrude surface. 0 is flat surface, 90 is when two faces
// are perpendicular
featureAngle 60;
// Maximum number of snapping relaxation iterations. Should stop
// before upon reaching a correct mesh.
nRelaxIter 5;
// Number of smoothing iterations of surface normals
nSmoothSurfaceNormals 1;
// Number of smoothing iterations of interior mesh movement direction
nSmoothNormals 3;
// Smooth layer thickness over surface patches
nSmoothThickness 10;
// Stop layer growth on highly warped cells
maxFaceThicknessRatio 0.5;
// Reduce layer growth where ratio thickness to medial
// distance is large
maxThicknessToMedialRatio 0.3;
// Angle used to pick up medial axis points
// Note: changed(corrected) w.r.t 17x! 90 degrees corresponds to 130 in 17x.
minMedianAxisAngle 90;
// Create buffer region for new layer terminations
nBufferCellsNoExtrude 0;
// Overall max number of layer addition iterations. The mesher will exit
// if it reaches this number of iterations; possibly with an illegal
// mesh.
nLayerIter 50;
// Max number of iterations after which relaxed meshQuality controls
// get used. Up to nRelaxIter it uses the settings in meshQualityControls,
// after nRelaxIter it uses the values in meshQualityControls::relaxed.
nRelaxedIter 20;
}
// Generic mesh quality settings. At any undoable phase these determine
// where to undo.
meshQualityControls
{
#include "meshQualityDict"
}
// Advanced
// Flags for optional output
// 0 : only write final meshes
// 1 : write intermediate meshes
// 2 : write volScalarField with cellLevel for postprocessing
// 4 : write current intersections as .obj files
debug 0;
// Merge tolerance. Is fraction of overall bounding box of initial mesh.
// Note: the write tolerance needs to be higher than this.
mergeTolerance 1E-6;
// ************************************************************************* //

48
tutorials/multiphase/interDyMFoam/ras/DTCHull/system/surfaceFeatureExtractDict Normal file
View File

@ -0,0 +1,48 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object surfaceFeatureExtractDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
DTC-scaled.stl
{
// How to obtain raw features (extractFromFile || extractFromSurface)
extractionMethod extractFromSurface;
extractFromSurfaceCoeffs
{
// Mark edges whose adjacent surface normals are at an angle less
// than includedAngle as features
// - 0 : selects no edges
// - 180: selects all edges
includedAngle 150;
}
subsetFeatures
{
// Keep nonManifold edges (edges with >2 connected faces)
nonManifoldEdges yes;
// Keep open edges (edges with 1 connected face)
openEdges yes;
}
// Write options
// Write features to obj format for postprocessing
writeObj yes;
}
// ************************************************************************* //

32
tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.1 Normal file
View File

@ -0,0 +1,32 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name c0;
type cellSet;
action new;
source boxToCell;
sourceInfo
{
box (-10 -6 -3) (10 0 3);
}
}
);
// ************************************************************************* //

32
tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.2 Normal file
View File

@ -0,0 +1,32 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name c0;
type cellSet;
action new;
source boxToCell;
sourceInfo
{
box (-5 -3 -2.5) (9 0 2);
}
}
);
// ************************************************************************* //

32
tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.3 Normal file
View File

@ -0,0 +1,32 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name c0;
type cellSet;
action new;
source boxToCell;
sourceInfo
{
box (-3 -1.5 -1) (8 0 1.5);
}
}
);
// ************************************************************************* //

32
tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.4 Normal file
View File

@ -0,0 +1,32 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name c0;
type cellSet;
action new;
source boxToCell;
sourceInfo
{
box (-2 -1 -0.6) (7 0 1);
}
}
);
// ************************************************************************* //

32
tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.5 Normal file
View File

@ -0,0 +1,32 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name c0;
type cellSet;
action new;
source boxToCell;
sourceInfo
{
box (-1 -0.6 -0.3) (6.5 0 0.8);
}
}
);
// ************************************************************************* //

32
tutorials/multiphase/interDyMFoam/ras/DTCHull/system/topoSetDict.6 Normal file
View File

@ -0,0 +1,32 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name c0;
type cellSet;
action new;
source boxToCell;
sourceInfo
{
box (-0.5 -0.55 -0.15) (6.25 0 0.65);
}
}
);
// ************************************************************************* //