zhyang-dev/OpenFOAM-12
1
0
Fork 0
Code Issues Pull Requests Actions Packages Projects Releases Wiki Activity

waves: Improved reverse flow formulation and new test cases

Browse Source 
It is now possible to use waveVelocity and waveAlpha boundary conditions
in cases in which the waves generate localised flow reversals along the
boundary. This means waves can be speficied at arbitrary directions and
with zero mean flow. Previously and integral approach, similar to
flowRateOutlet, was used, which was only correct when the direction of
wave propagation was aligned with the boundary normal.

This improvement has been achieved by reformulating the waveVelocity and
waveAlpha boundary conditions in terms of a new fixedValueInletOutlet
boundary condition type. This condition enforces a fixed value in all
cases except that of advection terms in the presence of outflow. In this
configuration a gradient condition is applied that will relax towards
the desired fixed value.

The wavePressure boundary condition has been removed, as it is no longer
necessary or advisable to locally switch between velocity and pressure
formulations along a wave boundary. Wave boundaries should now have the
general fixedFluxPressure or fixedFluxExtrapolatedPressure conditions
applied to the pressure field.

Two new tutorial cases have been created to demonstrate the new
functionality. The multiphase/interFoam/laminar/wave3D case demonstrates
wave generation with zero mean flow and at arbitrary angles to the
boundaries, and incompressible/pimpleFoam/RAS/waveSubSurface
demonstrates usage for sub-surface problems.
This commit is contained in:
Will Bainbridge
2021-09-01 10:55:23 +01:00
parent 984066f81e
commit 1c48685b09
54 changed files with 2213 additions and 711 deletions
Download Patch File Download Diff File Expand all files Collapse all files

43
tutorials/incompressible/pimpleFoam/RAS/waveSubSurface/0/U.orig Normal file
View File

@ -0,0 +1,43 @@
/*--------------------------------*- 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;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0 0 0);
boundaryField
{
bottom
{
type noSlip;
}
"(top|inlet)"
{
type waveVelocity;
}
outlet
{
type pressureInletOutletVelocity;
value $internalField;
}
"(front|back)"
{
type symmetryPlane;
}
}
// ************************************************************************* //

38
tutorials/incompressible/pimpleFoam/RAS/waveSubSurface/0/alpha.orig Normal file
View File

@ -0,0 +1,38 @@
/*--------------------------------*- 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 "0";
object alpha;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 0 0 0 0];
internalField uniform 1;
boundaryField
{
bottom
{
type zeroGradient;
}
"(top|inlet|outlet)"
{
type waveAlpha;
}
"(front|back)"
{
type symmetryPlane;
}
}
// ************************************************************************* //

41
tutorials/incompressible/pimpleFoam/RAS/waveSubSurface/0/epsilon Normal file
View File

@ -0,0 +1,41 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format binary;
class volScalarField;
location "0";
object epsilon;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -3 0 0 0 0];
internalField uniform 1.4e-6;
boundaryField
{
bottom
{
type epsilonWallFunction;
value $internalField;
}
"(top|inlet|outlet)"
{
type inletOutlet;
value $internalField;
inletValue $internalField;
}
"(front|back)"
{
type symmetryPlane;
}
}
// ************************************************************************* //

41
tutorials/incompressible/pimpleFoam/RAS/waveSubSurface/0/k Normal file
View File

@ -0,0 +1,41 @@
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format binary;
class volScalarField;
location "0";
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -2 0 0 0 0];
internalField uniform 1.4e-4;
boundaryField
{
bottom
{
type kqRWallFunction;
value $internalField;
}
"(top|inlet|outlet)"
{
type inletOutlet;
value $internalField;
inletValue $internalField;
}
"(front|back)"
{
type symmetryPlane;
}
}
// ************************************************************************* //

40
tutorials/incompressible/pimpleFoam/RAS/waveSubSurface/0/nut Normal file
View File

@ -0,0 +1,40 @@
/*--------------------------------*- 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 "0";
object nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -1 0 0 0 0];
internalField uniform 0;
boundaryField
{
bottom
{
type nutkWallFunction;
value uniform 0;
}
"(top|inlet|outlet)"
{
type calculated;
value $internalField;
}
"(front|back)"
{
type symmetryPlane;
}
}
// ************************************************************************* //

43
tutorials/incompressible/pimpleFoam/RAS/waveSubSurface/0/p Normal file
View File

@ -0,0 +1,43 @@
/*--------------------------------*- 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 "0";
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -2 0 0 0 0];
internalField uniform 0;
boundaryField
{
bottom
{
type fixedFluxPressure;
}
"(top|inlet)"
{
type fixedFluxExtrapolatedPressure;
}
outlet
{
type entrainmentPressure;
p0 $internalField;
value $internalField;
}
"(front|back)"
{
type symmetryPlane;
}
}
// ************************************************************************* //

13
tutorials/incompressible/pimpleFoam/RAS/waveSubSurface/Allrun Executable file
View File

@ -0,0 +1,13 @@
#!/bin/sh
cd ${0%/*} || exit 1
. $WM_PROJECT_DIR/bin/tools/RunFunctions
runApplication blockMesh
runApplication setWaves
runApplication decomposePar
runParallel $(getApplication)
runApplication reconstructPar -newTimes

21
tutorials/incompressible/pimpleFoam/RAS/waveSubSurface/constant/g Normal file
View File

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

27
tutorials/incompressible/pimpleFoam/RAS/waveSubSurface/constant/momentumTransport Normal file
View File

@ -0,0 +1,27 @@
/*--------------------------------*- 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 RAS;
RAS
{
RASModel kEpsilon;
turbulence on;
printCoeffs on;
}
// ************************************************************************* //

21
tutorials/incompressible/pimpleFoam/RAS/waveSubSurface/constant/physicalProperties Normal file
View File

@ -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;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
transportModel Newtonian;
nu [0 2 -1 0 0 0 0] 1e-05;
// ************************************************************************* //

38
tutorials/incompressible/pimpleFoam/RAS/waveSubSurface/constant/waveProperties Normal file
View File

@ -0,0 +1,38 @@
/*--------------------------------*- 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 waveProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
origin (0 0 2.7);
direction (1 0 0);
UMean (0 0 0);
waves
(
Stokes5
{
length 5.64;
amplitude 0.3;
phase 0.8;
angle 0;
depth 2.7;
}
);
scale table ((18 1) (24 0));
// ************************************************************************* //

96
tutorials/incompressible/pimpleFoam/RAS/waveSubSurface/system/blockMeshDict Normal file
View File

@ -0,0 +1,96 @@
/*--------------------------------*- 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 blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 1;
vertices
(
(0 -1.8 0) (0 1.8 0) (0 1.8 2) (0 -1.8 2)
(12 -1.8 0) (12 1.8 0) (12 1.8 2) (12 -1.8 2)
(24 -1.8 0) (24 1.8 0) (24 1.8 2) (24 -1.8 2)
);
blocks
(
hex (0 1 2 3 4 5 6 7) (20 24 72) simpleGrading (1 4 1)
hex (4 5 6 7 8 9 10 11) (20 24 24) simpleGrading (1 4 6)
);
edges
(
);
boundary
(
top
{
type patch;
faces
(
(2 3 7 6)
(6 7 11 10)
);
}
inlet
{
type patch;
faces
(
(0 1 2 3)
);
}
outlet
{
type patch;
faces
(
(8 9 10 11)
);
}
bottom
{
type wall;
faces
(
(0 1 5 4)
(4 5 9 8)
);
}
front
{
type symmetryPlane;
faces
(
(0 4 7 3)
(4 8 11 7)
);
}
back
{
type symmetryPlane;
faces
(
(1 5 6 2)
(5 9 10 6)
);
}
);
mergePatchPairs
(
);
// ************************************************************************* //

88
tutorials/incompressible/pimpleFoam/RAS/waveSubSurface/system/controlDict Normal file
View File

@ -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
{
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application pimpleFoam;
startFrom startTime;
startTime 0;
stopAt endTime;
endTime 100;
deltaT 0.01;
writeControl adjustableRunTime;
writeInterval 1;
purgeWrite 0;
writeFormat ascii;
writePrecision 10;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable yes;
adjustTimeStep no;
maxCo 1;
libs
(
"libwaves.so"
);
functions
{
readG
{
libs ("libutilityFunctionObjects.so");
type coded;
name readG;
enabled yes;
executeControl none;
codeRead
#{
if (!mesh().template foundObject<uniformDimensionedVectorField>("g"))
{
Info<< "\nReading g" << endl;
uniformDimensionedVectorField* g =
new uniformDimensionedVectorField
(
IOobject
(
"g",
mesh().time().constant(),
mesh(),
IOobject::MUST_READ,
IOobject::NO_WRITE
)
);
g->store();
}
#};
}
};
// ************************************************************************* //

29
tutorials/incompressible/pimpleFoam/RAS/waveSubSurface/system/decomposeParDict Normal file
View File

@ -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 "system";
object decomposeParDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
numberOfSubdomains 4;
method hierarchical;
hierarchicalCoeffs
{
n (4 1 1);
delta 0.001;
order xyz;
}
// ************************************************************************* //

58
tutorials/incompressible/pimpleFoam/RAS/waveSubSurface/system/fvSchemes Normal file
View File

@ -0,0 +1,58 @@
/*--------------------------------*- 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 linearUpwind grad(U);
div((nuEff*dev2(T(grad(U))))) Gauss linear;
div(U) Gauss linear;
div(phi,epsilon) Gauss limitedLinear 1;
div(phi,k) Gauss limitedLinear 1;
}
laplacianSchemes
{
default Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default corrected;
}
patchDist
{
method meshWave;
}
// ************************************************************************* //

58
tutorials/incompressible/pimpleFoam/RAS/waveSubSurface/system/fvSolution Normal file
View File

@ -0,0 +1,58 @@
/*--------------------------------*- 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-9;
relTol 0.01;
}
pFinal
{
$p;
relTol 0;
}
"(U|k|epsilon)"
{
solver PBiCGStab;
preconditioner DILU;
tolerance 1e-6;
relTol 0.1;
}
"(U|k|epsilon)Final"
{
$U;
relTol 0;
}
}
PIMPLE
{
nNonOrthogonalCorrectors 0;
nOuterCorrectors 2;
nCorrectors 1;
pRefCell 0;
pRefValue 0;
}
// ************************************************************************* //

20
tutorials/incompressible/pimpleFoam/RAS/waveSubSurface/system/setWavesDict Normal file
View File

@ -0,0 +1,20 @@
/*--------------------------------*- 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 setWavesDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
alpha alpha;
// ************************************************************************* //

41
tutorials/multiphase/interFoam/laminar/wave3D/0/U.orig Normal file
View File

@ -0,0 +1,41 @@
/*--------------------------------*- 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;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0 0 0);
boundaryField
{
#includeEtc "caseDicts/setConstraintTypes"
"(inlet|inletSide)"
{
type waveVelocity;
}
top
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
}
bottom
{
type noSlip;
}
}
// ************************************************************************* //

42
tutorials/multiphase/interFoam/laminar/wave3D/0/alpha.water.orig Normal file
View File

@ -0,0 +1,42 @@
/*--------------------------------*- 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 "0";
object alpha.water;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 0 0 0 0];
internalField uniform 0;
boundaryField
{
#includeEtc "caseDicts/setConstraintTypes"
"(inlet|inletSide)"
{
type waveAlpha;
}
top
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}
bottom
{
type zeroGradient;
}
}
// ************************************************************************* //

42
tutorials/multiphase/interFoam/laminar/wave3D/0/p_rgh Normal file
View File

@ -0,0 +1,42 @@
/*--------------------------------*- 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 "0";
object p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -2 0 0 0 0];
internalField uniform 0;
boundaryField
{
#includeEtc "caseDicts/setConstraintTypes"
"(inlet|inletSide)"
{
type fixedFluxPressure;
value uniform 0;
}
top
{
type entrainmentPressure;
p0 uniform 0;
}
bottom
{
type fixedFluxPressure;
value uniform 0;
}
}
// ************************************************************************* //

27
tutorials/multiphase/interFoam/laminar/wave3D/Allrun Executable file
View File

@ -0,0 +1,27 @@
#!/bin/sh
cd ${0%/*} || exit 1
. $WM_PROJECT_DIR/bin/tools/RunFunctions
runApplication blockMesh
for i in 1 2
do
runApplication -s XY$i topoSet -dict topoSetDictXY$i
runApplication -s XY$i refineMesh -dict refineMeshDictXY -overwrite
done
for i in 1 2 3 4
do
runApplication -s Z$i topoSet -dict topoSetDictZ$i
runApplication -s Z$i refineMesh -dict refineMeshDictZ -overwrite
done
runApplication setWaves
runApplication decomposePar
runParallel $(getApplication)
runApplication reconstructPar -newTimes

21
tutorials/multiphase/interFoam/laminar/wave3D/constant/g Normal file
View File

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

20
tutorials/multiphase/interFoam/laminar/wave3D/constant/momentumTransport Normal file
View File

@ -0,0 +1,20 @@
/*--------------------------------*- 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;
// ************************************************************************* //

22
tutorials/multiphase/interFoam/laminar/wave3D/constant/phaseProperties Normal file
View File

@ -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 phaseProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
phases (water air);
sigma 0;
// ************************************************************************* //

24
tutorials/multiphase/interFoam/laminar/wave3D/constant/physicalProperties.air Normal file
View File

@ -0,0 +1,24 @@
/*--------------------------------*- 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.air;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
viscosityModel constant;
nu 1.48e-05;
rho 1;
// ************************************************************************* //

24
tutorials/multiphase/interFoam/laminar/wave3D/constant/physicalProperties.water Normal file
View File

@ -0,0 +1,24 @@
/*--------------------------------*- 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.water;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
viscosityModel constant;
nu 1e-06;
rho 1000;
// ************************************************************************* //

39
tutorials/multiphase/interFoam/laminar/wave3D/constant/waveProperties Normal file
View File

@ -0,0 +1,39 @@
/*--------------------------------*- 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 waveProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
origin (0 0 0);
direction (1 0 0);
waves
(
Airy
{
length 300;
amplitude 2.5;
phase 0;
angle 0.5235987755982988;
}
);
UMean (0 0 0);
scale table ((1200 1) (1800 0));
crossScale table ((-1800 0) (-1200 1) (1200 1) (1800 0));
// ************************************************************************* //

112
tutorials/multiphase/interFoam/laminar/wave3D/system/blockMeshDict Normal file
View File

@ -0,0 +1,112 @@
/*--------------------------------*- 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 blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 1;
vertices
(
( 0 0 -300) (1200 0 -300) (2700 0 -300)
( 0 1200 -300) (1200 1200 -300) (2700 1200 -300)
( 0 2700 -300) (1200 2700 -300) (2700 2700 -300)
( 0 0 300) (1200 0 300) (2700 0 300)
( 0 1200 300) (1200 1200 300) (2700 1200 300)
( 0 2700 300) (1200 2700 300) (2700 2700 300)
);
blocks
(
hex (0 1 4 3 9 10 13 12) (67 67 40) simpleGrading (1 1 1)
hex (1 2 5 4 10 11 14 13) (27 67 40) simpleGrading (8 1 1)
hex (3 4 7 6 12 13 16 15) (67 27 40) simpleGrading (1 8 1)
hex (4 5 8 7 13 14 17 16) (27 27 40) simpleGrading (8 8 1)
);
edges
(
);
defaultPatch
{
name frontAndBack;
type empty;
}
boundary
(
inlet
{
type patch;
faces
(
(0 3 12 9)
(3 6 15 12)
);
}
inletSide
{
type patch;
faces
(
(0 1 10 9)
(1 2 11 10)
);
}
outletSide
{
type symmetryPlane;
faces
(
(6 7 16 15)
(7 8 17 16)
);
}
outlet
{
type symmetryPlane; //patch;
faces
(
(2 5 14 11)
(5 8 17 14)
);
}
bottom
{
type wall;
faces
(
(0 1 4 3)
(1 2 5 4)
(3 4 7 6)
(4 5 8 7)
);
}
top
{
type patch;
faces
(
(9 10 13 12)
(10 11 14 13)
(12 13 16 15)
(13 14 17 16)
);
}
);
// ************************************************************************* //

65
tutorials/multiphase/interFoam/laminar/wave3D/system/controlDict Normal file
View File

@ -0,0 +1,65 @@
/*--------------------------------*- 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 interFoam;
startFrom startTime;
startTime 0;
stopAt endTime;
endTime 100;
deltaT 0.05;
writeControl adjustableRunTime;
writeInterval 1;
purgeWrite 0;
writeFormat binary;
writePrecision 6;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable yes;
adjustTimeStep no;
maxCo 1;
maxAlphaCo 1;
maxDeltaT 1;
libs
(
"libwaves.so"
);
functions
{
#includeFunc isoSurface(isoField=alpha.water, isoValue=0.5, fields=())
}
// ************************************************************************* //

28
tutorials/multiphase/interFoam/laminar/wave3D/system/decomposeParDict Normal file
View File

@ -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 |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
location "system";
object decomposeParDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
numberOfSubdomains 18;
method hierarchical;
hierarchicalCoeffs
{
n (3 3 2);
order xyz;
}
// ************************************************************************* //

61
tutorials/multiphase/interFoam/laminar/wave3D/system/fvSchemes Normal file
View File

@ -0,0 +1,61 @@
/*--------------------------------*- 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 CrankNicolson ocCoeff
{
type scale;
scale linearRamp;
duration 1.0;
value 0.9;
};
*/
default Euler;
}
gradSchemes
{
default Gauss linear;
}
divSchemes
{
div(rhoPhi,U) Gauss linearUpwindV grad(U);
div(phi,alpha) Gauss interfaceCompression vanLeer 1;
div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default corrected;
}
// ************************************************************************* //

90
tutorials/multiphase/interFoam/laminar/wave3D/system/fvSolution Normal file
View File

@ -0,0 +1,90 @@
/*--------------------------------*- 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
{
"alpha.water.*"
{
nAlphaCorr 2;
nAlphaSubCycles 1;
MULESCorr yes;
nLimiterIter 3;
alphaApplyPrevCorr yes;
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-8;
relTol 0;
minIter 1;
}
pcorr
{
solver GAMG;
smoother DIC;
tolerance 1e-4;
relTol 0.01;
}
pcorrFinal
{
$pcorr;
relTol 0;
};
p_rgh
{
solver GAMG;
smoother DIC;
tolerance 1e-7;
relTol 0.001;
}
p_rghFinal
{
$p_rgh;
relTol 0;
}
"U.*"
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-7;
relTol 0;
}
}
PIMPLE
{
momentumPredictor yes;
nOuterCorrectors 1;
nCorrectors 3;
nNonOrthogonalCorrectors 0;
}
relaxationFactors
{
equations
{
".*" 1;
}
}
// ************************************************************************* //

40
tutorials/multiphase/interFoam/laminar/wave3D/system/refineMeshDictXY Normal file
View File

@ -0,0 +1,40 @@
/*--------------------------------*- 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 refineMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
set box;
coordinateSystem global;
globalCoeffs
{
e1 (1 0 0);
e2 (0 1 0);
}
directions
(
e1
e2
);
useHexTopology true;
geometricCut false;
writeMesh false;
// ************************************************************************* //

39
tutorials/multiphase/interFoam/laminar/wave3D/system/refineMeshDictZ Normal file
View File

@ -0,0 +1,39 @@
/*--------------------------------*- 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 refineMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
set box;
coordinateSystem global;
globalCoeffs
{
e1 (1 0 0);
e2 (0 1 0);
}
directions
(
e3
);
useHexTopology true;
geometricCut false;
writeMesh false;
// ************************************************************************* //

20
tutorials/multiphase/interFoam/laminar/wave3D/system/setWavesDict Normal file
View File

@ -0,0 +1,20 @@
/*--------------------------------*- 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 setWavesDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
alpha alpha.water;
// ************************************************************************* //

28
tutorials/multiphase/interFoam/laminar/wave3D/system/topoSetDictXY1 Normal file
View File

@ -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 |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
location "system";
object topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name box;
type cellSet;
action new;
source boxToCell;
box (-1e6 -1e6 -40) (1300 1300 40);
}
);
// ************************************************************************* //

28
tutorials/multiphase/interFoam/laminar/wave3D/system/topoSetDictXY2 Normal file
View File

@ -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 |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
location "system";
object topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name box;
type cellSet;
action new;
source boxToCell;
box (-1e6 -1e6 -30) (1200 1200 30);
}
);
// ************************************************************************* //

29
tutorials/multiphase/interFoam/laminar/wave3D/system/topoSetDictZ1 Normal file
View File

@ -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 "system";
object topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name box;
type cellSet;
action new;
source boxToCell;
//box (-1e6 -1e6 -40) (1500 1500 40);
box (-1e6 -1e6 -40) (1e6 1e6 40);
}
);
// ************************************************************************* //

29
tutorials/multiphase/interFoam/laminar/wave3D/system/topoSetDictZ2 Normal file
View File

@ -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 "system";
object topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name box;
type cellSet;
action new;
source boxToCell;
//box (-1e6 -1e6 -30) (1400 1400 30);
box (-1e6 -1e6 -30) (1e6 1e6 30);
}
);
// ************************************************************************* //

29
tutorials/multiphase/interFoam/laminar/wave3D/system/topoSetDictZ3 Normal file
View File

@ -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 "system";
object topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name box;
type cellSet;
action new;
source boxToCell;
//box (-1e6 -1e6 -20) (1300 1300 20);
box (-1e6 -1e6 -20) (1e6 1e6 20);
}
);
// ************************************************************************* //

29
tutorials/multiphase/interFoam/laminar/wave3D/system/topoSetDictZ4 Normal file
View File

@ -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 "system";
object topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name box;
type cellSet;
action new;
source boxToCell;
//box (-1e6 -1e6 -10) (1200 1200 10);
box (-1e6 -1e6 -10) (1e6 1e6 10);
}
);
// ************************************************************************* //