zhyang-dev/OpenFOAM-5.x
1
0
Fork 0
Code Issues Pull Requests Actions Packages Projects Releases Wiki Activity

tutorials: interFoam: Added 2D wave propagation case

Browse Source
This commit is contained in:
Will Bainbridge
2017-05-30 09:58:42 +01:00
parent e7e4683f96
commit 2aa78c6db3
24 changed files with 994 additions and 0 deletions
Download Patch File Download Diff File Expand all files Collapse all files

63
tutorials/multiphase/interFoam/laminar/wave/0.org/U 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 volVectorField;
location "0";
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0 0 0);
boundaryField
{
#includeEtc "caseDicts/setConstraintTypes"
left
{
type waveVelocity;
origin (0 0 0);
direction (1 0 0);
speed 2;
waves
(
Airy
{
length 300;
amplitude 2.5;
phase 0;
angle 0;
}
);
scale table ((1200 1) (1800 0));
crossScale constant 1;
}
right
{
type outletPhaseMeanVelocity;
Umean 2;
alpha alpha.water;
}
top
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
}
bottom
{
type noSlip;
}
}
// ************************************************************************* //

45
tutorials/multiphase/interFoam/laminar/wave/0.org/alpha.water Normal file
View File

@ -0,0 +1,45 @@
/*--------------------------------*- 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.water;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 0 0 0 0];
internalField uniform 0;
boundaryField
{
#includeEtc "caseDicts/setConstraintTypes"
"(right|bottom)"
{
type zeroGradient;
}
left
{
type waveAlpha;
U U;
inletOutlet true;
}
top
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}
}
// ************************************************************************* //

38
tutorials/multiphase/interFoam/laminar/wave/0.org/p_rgh Normal file
View File

@ -0,0 +1,38 @@
/*--------------------------------*- 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
{
#includeEtc "caseDicts/setConstraintTypes"
"(left|right|bottom)"
{
type fixedFluxPressure;
value uniform 0;
}
top
{
type totalPressure;
p0 uniform 0;
}
}
// ************************************************************************* //

7
tutorials/multiphase/interFoam/laminar/wave/Allclean Executable file
View File

@ -0,0 +1,7 @@
#!/bin/sh
cd ${0%/*} || exit 1
. $WM_PROJECT_DIR/bin/tools/CleanFunctions
cleanCase && rm -rf 0

33
tutorials/multiphase/interFoam/laminar/wave/Allrun Executable file
View File

@ -0,0 +1,33 @@
#!/bin/sh
cd ${0%/*} || exit 1
. $WM_PROJECT_DIR/bin/tools/RunFunctions
runApplication blockMesh
cp -r 0.org 0
runApplication extrudeMesh
for i in 1 2
do
runApplication -s $i topoSet -dict system/topoSetDict$i
runApplication -s $i refineMesh -dict system/refineMeshDictX -overwrite
done
for i in 3 4 5 6
do
runApplication -s $i topoSet -dict system/topoSetDict$i
runApplication -s $i refineMesh -dict system/refineMeshDictY -overwrite
done
runApplication topoSet
runApplication setWaves -alpha alpha.water
runApplication decomposePar
runParallel $(getApplication)
runApplication reconstructPar

32
tutorials/multiphase/interFoam/laminar/wave/constant/fvOptions Normal file
View File

@ -0,0 +1,32 @@
/*--------------------------------*- 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 fvOptions;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
option1
{
type verticalDamping;
selectionMode cellZone;
cellZone right;
lambda 0.1;
timeStart 0;
duration 1e6;
}
//************************************************************************* //

22
tutorials/multiphase/interFoam/laminar/wave/constant/g Normal file
View File

@ -0,0 +1,22 @@
/*--------------------------------*- 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 -9.81 0);
// ************************************************************************* //

37
tutorials/multiphase/interFoam/laminar/wave/constant/transportProperties Normal file
View File

@ -0,0 +1,37 @@
/*--------------------------------*- 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 1e-06;
rho 1000;
}
air
{
transportModel Newtonian;
nu 1.48e-05;
rho 1;
}
sigma 0;
// ************************************************************************* //

21
tutorials/multiphase/interFoam/laminar/wave/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 laminar;
// ************************************************************************* //

88
tutorials/multiphase/interFoam/laminar/wave/system/blockMeshDict Normal file
View File

@ -0,0 +1,88 @@
/*--------------------------------*- 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 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)
);
edges
(
);
defaultPatch
{
name frontAndBack;
type empty;
}
boundary
(
left
{
type patch;
faces
(
(0 4 7 3)
);
}
right
{
type patch;
faces
(
(2 6 5 1)
);
}
bottom
{
type patch;
faces
(
(0 1 5 4)
);
}
top
{
type patch;
faces
(
(2 3 7 6)
);
}
);
mergePatchPairs
(
);
// ************************************************************************* //

72
tutorials/multiphase/interFoam/laminar/wave/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 interFoam;
startFrom startTime;
startTime 0;
stopAt endTime;
endTime 200;
deltaT 0.05;
writeControl adjustableRunTime;
writeInterval 1;
purgeWrite 0;
writeFormat binary;
writePrecision 6;
writeCompression uncompressed;
timeFormat general;
timePrecision 6;
runTimeModifiable yes;
adjustTimeStep no;
maxCo 1;
maxAlphaCo 1;
maxDeltaT 1;
libs
(
"libwaves.so"
);
functions
{
interfaceHeight1
{
type interfaceHeight;
libs ("libfieldFunctionObjects.so");
locations ((300 0 0) (450 0 0) (600 0 0));
alpha alpha.water;
}
}
// ************************************************************************* //

29
tutorials/multiphase/interFoam/laminar/wave/system/decomposeParDict Normal file
View File

@ -0,0 +1,29 @@
/*--------------------------------*- 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 decomposeParDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
numberOfSubdomains 6;
method simple;
simpleCoeffs
{
n (3 2 1);
delta 0.001;
}
// ************************************************************************* //

40
tutorials/multiphase/interFoam/laminar/wave/system/extrudeMeshDict Normal file
View File

@ -0,0 +1,40 @@
/*--------------------------------*- 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 extrudeMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
constructFrom mesh;
sourceCase ".";
sourcePatches (right);
flipNormals false;
nLayers 25;
expansionRatio 1.09;
extrudeModel linearNormal;
linearNormalCoeffs
{
thickness 1500;
}
mergeFaces false;
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

58
tutorials/multiphase/interFoam/laminar/wave/system/fvSchemes 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 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 vanLeer;
div(phirb,alpha) Gauss linear;
div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default corrected;
}
// ************************************************************************* //

95
tutorials/multiphase/interFoam/laminar/wave/system/fvSolution Normal file
View File

@ -0,0 +1,95 @@
/*--------------------------------*- 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 25;
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/wave/system/refineMeshDictX Normal file
View File

@ -0,0 +1,40 @@
/*--------------------------------*- 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 refineMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
set box;
coordinateSystem global;
globalCoeffs
{
tan1 (1 0 0);
tan2 (0 1 0);
}
directions
(
tan1
);
useHexTopology true;
geometricCut false;
writeMesh false;
// ************************************************************************* //

40
tutorials/multiphase/interFoam/laminar/wave/system/refineMeshDictY Normal file
View File

@ -0,0 +1,40 @@
/*--------------------------------*- 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 refineMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
set box;
coordinateSystem global;
globalCoeffs
{
tan1 (1 0 0);
tan2 (0 1 0);
}
directions
(
tan2
);
useHexTopology true;
geometricCut false;
writeMesh false;
// ************************************************************************* //

42
tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict Normal file
View File

@ -0,0 +1,42 @@
/*--------------------------------*- 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 topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name right;
type cellSet;
action new;
source boxToCell;
sourceInfo
{
box (1800 -1e6 -1e6) (1e6 1e6 1e6);
}
}
{
name right;
type cellZoneSet;
action new;
source setToCellZone;
sourceInfo
{
set right;
}
}
);
// ************************************************************************* //

32
tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict1 Normal file
View File

@ -0,0 +1,32 @@
/*--------------------------------*- 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 topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name box;
type cellSet;
action new;
source boxToCell;
sourceInfo
{
box (-1e6 -40 -1e6) (1300 40 1e6);
}
}
);
// ************************************************************************* //

32
tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict2 Normal file
View File

@ -0,0 +1,32 @@
/*--------------------------------*- 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 topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name box;
type cellSet;
action new;
source boxToCell;
sourceInfo
{
box (-1e6 -30 -1e6) (1200 30 1e6);
}
}
);
// ************************************************************************* //

32
tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict3 Normal file
View File

@ -0,0 +1,32 @@
/*--------------------------------*- 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 topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name box;
type cellSet;
action new;
source boxToCell;
sourceInfo
{
box (-1e6 -40 -1e6) (1e6 40 1e6);
}
}
);
// ************************************************************************* //

32
tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict4 Normal file
View File

@ -0,0 +1,32 @@
/*--------------------------------*- 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 topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name box;
type cellSet;
action new;
source boxToCell;
sourceInfo
{
box (-1e6 -30 -1e6) (1e6 30 1e6);
}
}
);
// ************************************************************************* //

32
tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict5 Normal file
View File

@ -0,0 +1,32 @@
/*--------------------------------*- 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 topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name box;
type cellSet;
action new;
source boxToCell;
sourceInfo
{
box (-1e6 -20 -1e6) (1e6 20 1e6);
}
}
);
// ************************************************************************* //

32
tutorials/multiphase/interFoam/laminar/wave/system/topoSetDict6 Normal file
View File

@ -0,0 +1,32 @@
/*--------------------------------*- 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 topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name box;
type cellSet;
action new;
source boxToCell;
sourceInfo
{
box (-1e6 -10 -1e6) (1e6 10 1e6);
}
}
);
// ************************************************************************* //