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

fvModels::waveForcing: New fvModel to generate VoF surface by region forcing

Browse Source 
With waveForcing waves can be generated with a domain by applying forcing to
both the phase-fraction and velocity fields rather than requiring that the waves
are introduced at an inlet.  This provides much greater flexibility as waves can
be generated in any direction relative to the mean flow, obliquely or even
against the flow.  isotropicDamping or verticalDamping can be used in
conjunction with waveForcing to damp the waves before they reach an outlet,
alternatively waveForcing can be used in regions surrounding a hull for example
to maintain far-field waves everywhere.

The tutorials/multiphase/interFoam/laminar/forcedWave tutorial case is provided
to demonstrate the waveForcing fvModel as an alternative to the wave inlet
boundary conditions used in the tutorials/multiphase/interFoam/laminar/wave
case.

Class
    Foam::fv::waveForcing

Description
    This fvModel applies forcing to the liquid phase-fraction field and all
    components of the vector field to relax the fields towards those
    calculated from the current wave distribution.

    The forcing force coefficient \f$\lambda\f$ should be set based on the
    desired level of forcing and the residence time the waves through the
    forcing zone.  For example, if waves moving at 2 [m/s] are travelling
    through a forcing zone 8 [m] in length, then the residence time is 4 [s]. If
    it is deemed necessary to force for 5 time-scales, then \f$\lambda\f$ should
    be set to equal 5/(4 [s]) = 1.2 [1/s].

Usage
    Example usage:
    \verbatim
    waveForcing1
    {
        type            waveForcing;

        libs            ("libwaves.so");

        liquidPhase     water;

        // Define the line along which to apply the graduation
        origin          (600 0 0);
        direction       (-1 0 0);

        // // Or, define multiple lines
        // origins         ((600 0 0) (600 -300 0) (600 300 0));
        // directions      ((-1 0 0) (0 1 0) (0 -1 0));

        scale
        {
            type        halfCosineRamp;
            start       0;
            duration    300;
        }

        lambda          0.5; // Forcing coefficient
    }
    \endverbatim
This commit is contained in:
Henry Weller
2022-10-03 20:30:02 +01:00
parent 9dc91eb479
commit 562925476b
38 changed files with 1512 additions and 59 deletions
Download Patch File Download Diff File Expand all files Collapse all files

49
tutorials/multiphase/interFoam/laminar/forcedWave/0/U.orig Normal file
View File

@ -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 volVectorField;
location "0";
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];
internalField uniform (2 0 0);
boundaryField
{
#includeEtc "caseDicts/setConstraintTypes"
left
{
type fixedValue;
value $internalField;
}
right
{
type outletPhaseMeanVelocity;
UnMean 2;
alpha alpha.water;
}
top
{
type pressureInletOutletVelocity;
tangentialVelocity $internalField;
value $internalField;
}
bottom
{
type noSlip;
}
}
// ************************************************************************* //

43
tutorials/multiphase/interFoam/laminar/forcedWave/0/alpha.water.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 volScalarField;
location "0";
object alpha.water;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 0 0 0 0];
internalField uniform 0;
boundaryField
{
#includeEtc "caseDicts/setConstraintTypes"
"(right|bottom)"
{
type zeroGradient;
}
left
{
type fixedValue;
value $internalField;
}
top
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}
}
// ************************************************************************* //

38
tutorials/multiphase/interFoam/laminar/forcedWave/0/p_rgh 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 p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -2 0 0 0 0];
internalField uniform 0;
boundaryField
{
#includeEtc "caseDicts/setConstraintTypes"
"(left|right|bottom)"
{
type fixedFluxPressure;
value uniform 0;
}
top
{
type prghTotalPressure;
p0 uniform 0;
}
}
// ************************************************************************* //

29
tutorials/multiphase/interFoam/laminar/forcedWave/Allrun Executable file
View File

@ -0,0 +1,29 @@
#!/bin/sh
cd ${0%/*} || exit 1
. $WM_PROJECT_DIR/bin/tools/RunFunctions
runApplication blockMesh
runApplication extrudeMesh
for i in 1 2
do
runApplication -s $i topoSet -dict topoSetDict$i
runApplication -s $i refineMesh -dict refineMeshDictX -overwrite
done
for i in 3 4 5 6
do
runApplication -s $i topoSet -dict topoSetDict$i
runApplication -s $i refineMesh -dict refineMeshDictY -overwrite
done
runApplication setFields
runApplication decomposePar
runParallel $(getApplication)
runApplication reconstructPar

60
tutorials/multiphase/interFoam/laminar/forcedWave/constant/fvModels Normal file
View File

@ -0,0 +1,60 @@
/*--------------------------------*- 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;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
forcing
{
type waveForcing;
libs ("libwaves.so");
liquidPhase water;
origin (600 0 0);
direction (-1 0 0);
scale
{
type halfCosineRamp;
start 0;
duration 300;
}
lambda 0.5;
}
damping
{
type isotropicDamping;
libs ("libwaves.so");
origin (1200 0 0);
direction (1 0 0);
scale
{
type halfCosineRamp;
start 0;
duration 600;
}
lambda 0.5;
value (2 0 0);
}
//************************************************************************* //

34
tutorials/multiphase/interFoam/laminar/forcedWave/constant/fvModels.verticalDamping Normal file
View File

@ -0,0 +1,34 @@
/*--------------------------------*- 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;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
option1
{
type verticalDamping;
origin (1200 0 0);
direction (1 0 0);
scale
{
type halfCosineRamp;
start 0;
duration 600;
}
lambda 0.5;
}
//************************************************************************* //

21
tutorials/multiphase/interFoam/laminar/forcedWave/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 -9.81 0);
// ************************************************************************* //

20
tutorials/multiphase/interFoam/laminar/forcedWave/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/forcedWave/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/forcedWave/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/forcedWave/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;
// ************************************************************************* //

35
tutorials/multiphase/interFoam/laminar/forcedWave/constant/waveProperties Normal file
View File

@ -0,0 +1,35 @@
/*--------------------------------*- 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;
}
);
UMean (2 0 0);
// ************************************************************************* //

80
tutorials/multiphase/interFoam/laminar/forcedWave/system/blockMeshDict Normal file
View File

@ -0,0 +1,80 @@
/*--------------------------------*- 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 -300 -10)
(1200 -300 -10)
(1200 300 -10)
(0 300 -10)
(0 -300 10)
(1200 -300 10)
(1200 300 10)
(0 300 10)
);
blocks
(
hex (0 1 2 3 4 5 6 7) (67 40 1) simpleGrading (1 1 1)
);
defaultPatch
{
name frontAndBack;
type empty;
}
boundary
(
left
{
type patch;
faces
(
(0 4 7 3)
);
}
right
{
type patch;
faces
(
(2 6 5 1)
);
}
bottom
{
type wall;
faces
(
(0 1 5 4)
);
}
top
{
type patch;
faces
(
(2 3 7 6)
);
}
);
// ************************************************************************* //

66
tutorials/multiphase/interFoam/laminar/forcedWave/system/controlDict Normal file
View File

@ -0,0 +1,66 @@
/*--------------------------------*- 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 200;
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;
functions
{
interfaceHeight1
{
type interfaceHeight;
libs ("libfieldFunctionObjects.so");
locations ((300 0 0) (450 0 0) (600 0 0));
alpha alpha.water;
}
}
// ************************************************************************* //

27
tutorials/multiphase/interFoam/laminar/forcedWave/system/decomposeParDict 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 "system";
object decomposeParDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
numberOfSubdomains 6;
method simple;
simpleCoeffs
{
n (3 2 1);
}
// ************************************************************************* //

39
tutorials/multiphase/interFoam/laminar/forcedWave/system/extrudeMeshDict 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 extrudeMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
constructFrom mesh;
sourceCase ".";
sourcePatches (right);
flipNormals false;
nLayers 25;
expansionRatio 1.09;
extrudeModel linearNormal;
linearNormalCoeffs
{
thickness 1500;
}
mergeFaces false;
// ************************************************************************* //

57
tutorials/multiphase/interFoam/laminar/forcedWave/system/fvSchemes Normal file
View File

@ -0,0 +1,57 @@
/*--------------------------------*- 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;
};
}
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/forcedWave/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;
}
}
// ************************************************************************* //

39
tutorials/multiphase/interFoam/laminar/forcedWave/system/refineMeshDictX 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
(
e1
);
useHexTopology true;
geometricCut false;
writeMesh false;
// ************************************************************************* //

39
tutorials/multiphase/interFoam/laminar/forcedWave/system/refineMeshDictY 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
(
e2
);
useHexTopology true;
geometricCut false;
writeMesh false;
// ************************************************************************* //

47
tutorials/multiphase/interFoam/laminar/forcedWave/system/setFieldsDict Normal file
View File

@ -0,0 +1,47 @@
/*--------------------------------*- 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 setFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
defaultFieldValues
(
volScalarFieldValue alpha.water 0
);
regions
(
boxToCell
{
box (-10000 -10000 -10000) (10000 0 10000);
fieldValues
(
volScalarFieldValue alpha.water 1
);
}
// Set patch values (using ==)
boxToFace
{
box (-10000 -10000 -10000) (10000 0 10000);
fieldValues
(
volScalarFieldValue alpha.water 1
);
}
);
// ************************************************************************* //

19
tutorials/multiphase/interFoam/laminar/forcedWave/system/setWavesDict Normal file
View File

@ -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;
object setWavesDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
alpha alpha.water;
// ************************************************************************* //

28
tutorials/multiphase/interFoam/laminar/forcedWave/system/topoSetDict1 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 -40 -1e6) (1300 40 1e6);
}
);
// ************************************************************************* //

28
tutorials/multiphase/interFoam/laminar/forcedWave/system/topoSetDict2 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 -30 -1e6) (1200 30 1e6);
}
);
// ************************************************************************* //

28
tutorials/multiphase/interFoam/laminar/forcedWave/system/topoSetDict3 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 -40 -1e6) (1e6 40 1e6);
}
);
// ************************************************************************* //

28
tutorials/multiphase/interFoam/laminar/forcedWave/system/topoSetDict4 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 -30 -1e6) (1e6 30 1e6);
}
);
// ************************************************************************* //

28
tutorials/multiphase/interFoam/laminar/forcedWave/system/topoSetDict5 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 -20 -1e6) (1e6 20 1e6);
}
);
// ************************************************************************* //

28
tutorials/multiphase/interFoam/laminar/forcedWave/system/topoSetDict6 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 -10 -1e6) (1e6 10 1e6);
}
);
// ************************************************************************* //