zhyang-dev/openfoam
1
0
Fork 0
mirror of https://develop.openfoam.com/Development/openfoam.git synced 2025-11-28 03:28:01 +00:00
Code Issues Actions Packages Projects Releases Wiki Activity

Template case files to help general setup of OpenFOAM cases

Browse Source 
The templates include a stategy to simplify meshing with snappyHexMesh,
particularly to help generate an initial mesh quickly that can subsequently be
improved.  The templates are setup to enable rapid initial simulations, typically
with simpleFoam.  The initial templates cover simple inflow-outflow and closed
domains, including rotating geometry, and an example axisymmetric flow.  For
more details, consult the README file accompanying each template case.
The cases are located in $FOAM_ETC/templates
This commit is contained in:
Chris Greenshields
2015-05-18 18:34:01 +01:00
parent 93b3113b04
commit 6f82273f8c
101 changed files with 4394 additions and 0 deletions
Download Patch File Download Diff File Expand all files Collapse all files

46
etc/templates/inflowOutflow/0/U Normal file
View File

@ -0,0 +1,46 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volVectorField;
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Uinlet (10 0 0);
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0 0 0);
boundaryField
{
inlet
{
type fixedValue;
value uniform $Uinlet;
}
outlet
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
}
wall
{
type fixedValue;
value uniform (0 0 0);
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //

47
etc/templates/inflowOutflow/0/k Normal file
View File

@ -0,0 +1,47 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
kInlet 0.1;
dimensions [0 2 -2 0 0 0 0];
internalField uniform $kInlet;
boundaryField
{
inlet
{
type fixedValue;
value uniform $kInlet;
}
outlet
{
type inletOutlet;
inletValue uniform $kInlet;
value uniform $kInlet;
}
wall
{
type kqRWallFunction;
value uniform $kInlet;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //

44
etc/templates/inflowOutflow/0/nut Normal file
View File

@ -0,0 +1,44 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -1 0 0 0 0];
internalField uniform 0;
boundaryField
{
inlet
{
type calculated;
value uniform 0;
}
outlet
{
type calculated;
value uniform 0;
}
wall
{
type nutkWallFunction;
value uniform 0;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //

47
etc/templates/inflowOutflow/0/omega Normal file
View File

@ -0,0 +1,47 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object omega;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
omegaInlet 1.0;
dimensions [0 0 -1 0 0 0 0];
internalField uniform $omegaInlet;
boundaryField
{
inlet
{
type fixedValue;
value uniform $omegaInlet;
}
outlet
{
type inletOutlet;
inletValue uniform $omegaInlet;
value uniform $omegaInlet;
}
wall
{
type omegaWallFunction;
value uniform $omegaInlet;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //

42
etc/templates/inflowOutflow/0/p 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 volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -2 0 0 0 0];
internalField uniform 0;
boundaryField
{
inlet
{
type zeroGradient;
}
outlet
{
type fixedValue;
value uniform 0;
}
wall
{
type zeroGradient;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //

54
etc/templates/inflowOutflow/README Normal file
View File

@ -0,0 +1,54 @@
Overview
========
+ This is a template case with single inlet and outlet
+ Setup to run the simpleFoam solver
+ The case is designed to be meshed with snappyHexMesh
+ snappyHexMesh is setup to use a single trisurface file named CAD.obj
+ Copy the CAD.obj file to the constant/triSurface directory
+ The CAD.obj should contain an inlet and outlet region to create the relevant
patches in the mesh
Background Mesh
===============
+ The user should establish the bounds of their CAD.obj file
+ The blockMeshDict file contains a backgroundMesh subditionary
+ Set xMin, xMax, etc to be beyond the CAD.obj bounds
+ Set background mesh density with xCells, yCells, zCells
+ Run blockMesh
Background Mesh (alternative)
=============================
+ The user can adopt the background mesh patches in the mesh
+ For example, the background mesh can provide external patches of an external
flow
+ An alternative blockMeshDict file is set up for this: blockMeshDict.extPatches
+ Simply copy blockMeshDict.extPatches to blockMeshDict and edit inlet, outlet
patches accordingly
Castellated Mesh
================
+ In the snappyHexMeshDict file, replace <inletPatch> with the name of the inlet
region in the CAD.obj file
+ Replace <outletPatch> with the name of the outlet region
+ run snappyHexMesh to obtain a castellatedMesh
+ Review the mesh; modify refinement levels and regenerate the mesh as required
(levels are set in refinementSurfaces and refinementRegions)
Snapped Mesh
============
+ In snappyHexMeshDict, set castellatedMesh off; snap on;
+ Run the snapping phase of snappyHexMesh
+ Review the mesh
Layers
======
+ To add layers to the mesh along wall boundary patches...
+ Switch on addLayers; switch snap off;
+ Run snappyHexMesh
+ The number of layers can be changed by modifying nSurfaceLayers
Initialisation
==============
+ In the field files in the 0 directory, set inlet values
+ For example, in 0/U, set the inlet velocity Uinlet
+ Set the viscosity in constant/transportProperties

23
etc/templates/inflowOutflow/constant/RASProperties Normal file
View File

@ -0,0 +1,23 @@
/*--------------------------------*- 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 RASProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
RASModel kOmegaSST;
turbulence on;
printCoeffs on;
// ************************************************************************* //

68
etc/templates/inflowOutflow/constant/polyMesh/blockMeshDict Normal file
View File

@ -0,0 +1,68 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
backgroundMesh
{
xMin -1;
xMax 1;
yMin -1;
yMax 1;
zMin -1;
zMax 1;
xCells 20;
yCells 20;
zCells 20;
}
convertToMeters 1;
vertices
(
($:backgroundMesh.xMin $:backgroundMesh.yMin $:backgroundMesh.zMin)
($:backgroundMesh.xMax $:backgroundMesh.yMin $:backgroundMesh.zMin)
($:backgroundMesh.xMax $:backgroundMesh.yMax $:backgroundMesh.zMin)
($:backgroundMesh.xMin $:backgroundMesh.yMax $:backgroundMesh.zMin)
($:backgroundMesh.xMin $:backgroundMesh.yMin $:backgroundMesh.zMax)
($:backgroundMesh.xMax $:backgroundMesh.yMin $:backgroundMesh.zMax)
($:backgroundMesh.xMax $:backgroundMesh.yMax $:backgroundMesh.zMax)
($:backgroundMesh.xMin $:backgroundMesh.yMax $:backgroundMesh.zMax)
);
blocks
(
hex (0 1 2 3 4 5 6 7)
(
$:backgroundMesh.xCells
$:backgroundMesh.yCells
$:backgroundMesh.zCells
)
simpleGrading (1 1 1)
);
edges
(
);
boundary
(
);
mergePatchPairs
(
);
// ************************************************************************* //

121
etc/templates/inflowOutflow/constant/polyMesh/blockMeshDict.extPatches Normal file
View File

@ -0,0 +1,121 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
backgroundMesh
{
xMin -1;
xMax 1;
yMin -1;
yMax 1;
zMin -1;
zMax 1;
xCells 20;
yCells 20;
zCells 20;
}
convertToMeters 1;
vertices
(
($:backgroundMesh.xMin $:backgroundMesh.yMin $:backgroundMesh.zMin)
($:backgroundMesh.xMax $:backgroundMesh.yMin $:backgroundMesh.zMin)
($:backgroundMesh.xMax $:backgroundMesh.yMax $:backgroundMesh.zMin)
($:backgroundMesh.xMin $:backgroundMesh.yMax $:backgroundMesh.zMin)
($:backgroundMesh.xMin $:backgroundMesh.yMin $:backgroundMesh.zMax)
($:backgroundMesh.xMax $:backgroundMesh.yMin $:backgroundMesh.zMax)
($:backgroundMesh.xMax $:backgroundMesh.yMax $:backgroundMesh.zMax)
($:backgroundMesh.xMin $:backgroundMesh.yMax $:backgroundMesh.zMax)
);
blocks
(
hex (0 1 2 3 4 5 6 7)
(
$:backgroundMesh.xCells
$:backgroundMesh.yCells
$:backgroundMesh.zCells
)
simpleGrading (1 1 1)
);
edges
(
);
boundary
(
left
{
type patch;
faces
(
(0 3 7 4)
);
}
right
{
type patch;
faces
(
(1 5 6 2)
);
}
bottom
{
type patch;
faces
(
(0 1 2 3)
);
}
top
{
type patch;
faces
(
(4 7 6 5)
);
}
back
{
type patch;
faces
(
(0 4 5 1)
);
}
front
{
type patch;
faces
(
(3 2 6 7)
);
}
);
mergePatchPairs
(
);
// ************************************************************************* //

21
etc/templates/inflowOutflow/constant/transportProperties 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;
object transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
transportModel Newtonian;
nu nu [ 0 2 -1 0 0 0 0 ] 1.5e-05;
// ************************************************************************* //

0
etc/templates/inflowOutflow/constant/triSurface/.keep Normal file
View File

19
etc/templates/inflowOutflow/constant/turbulenceProperties Normal file
View File

@ -0,0 +1,19 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
simulationType RASModel;
// ************************************************************************* //

55
etc/templates/inflowOutflow/system/controlDict Normal file
View File

@ -0,0 +1,55 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application simpleFoam;
startFrom latestTime;
startTime 0;
stopAt endTime;
endTime 1000;
deltaT 1;
writeControl timeStep;
writeInterval 50;
purgeWrite 0;
writeFormat ascii;
writePrecision 8;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable true;
// adjustTimeStep yes;
// maxCo 1;
functions
{
}
// ************************************************************************* //

67
etc/templates/inflowOutflow/system/fvSchemes 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 fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
default steadyState;
}
gradSchemes
{
default Gauss linear;
limited cellLimited Gauss linear 1;
grad(U) $limited;
grad(k) $limited;
grad(omega) $limited;
}
divSchemes
{
default none;
div(phi,U) bounded Gauss linearUpwind limited;
turbulence bounded Gauss limitedLinear 1;
div(phi,k) $turbulence;
div(phi,omega) $turbulence;
div(phi,epsilon) $turbulence;
div((nuEff*dev(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default corrected;
}
fluxRequired
{
default no;
p ;
}
// ************************************************************************* //

93
etc/templates/inflowOutflow/system/fvSolution Normal file
View File

@ -0,0 +1,93 @@
/*--------------------------------*- 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 fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
p
{
solver GAMG;
smoother GaussSeidel;
cacheAgglomeration on; // Need to make this default?
agglomerator faceAreaPair; // Need to make this default?
nCellsInCoarsestLevel 10; // Need to make this default?
mergeLevels 1; // Need to make this default
tolerance 1e-6;
relTol 0.1;
}
"(U|k|omega|epsilon)"
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-6;
relTol 0.1;
}
pFinal
{
$p;
relTol 0;
}
"(U|k|omega|epsilon)Final"
{
$U;
relTol 0;
}
}
"(PIMPLE|PISO)"
{
nOuterCorrectors 1;
nCorrectors 2;
nNonOrthogonalCorrectors 1;
pRefCell 0;
pRefValue 0;
}
SIMPLE
{
residualControl
{
p 1e-4;
U 1e-4;
"(k|omega|epsilon)" 1e-4;
}
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;
}
potentialFlow
{
nNonOrthogonalCorrectors 10;
}
relaxationFactors
{
fields
{
p 0.3;
}
equations
{
U 0.7;
"(k|omega|epsilon)" 0.7;
}
}
// ************************************************************************* //

22
etc/templates/inflowOutflow/system/meshQualityDict 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 dictionary;
object meshQualityDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#includeEtc "caseDicts/mesh/generation/meshQualityDict.cfg"
//- minFaceWeight (0 -> 0.5)
//minFaceWeight 0.02;
// ************************************************************************* //

120
etc/templates/inflowOutflow/system/snappyHexMeshDict Normal file
View File

@ -0,0 +1,120 @@
/*--------------------------------*- 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;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#includeEtc "caseDicts/mesh/generation/snappyHexMeshDict.cfg"
castellatedMesh on;
snap off;
addLayers off;
geometry
{
CAD.obj
{
type triSurfaceMesh;
name CAD;
regions
{
<inletPatch> { name inlet; }
<outletPatch> { name outlet; }
}
}
};
castellatedMeshControls
{
features
(
// { file "CAD.eMesh"; level 1; }
);
refinementSurfaces
{
CAD
{
level (2 2);
patchInfo { type wall; }
regions
{
<inletPatch>
{
level (2 2);
patchInfo { type patch; }
}
<outletPatch>
{
level (2 2);
patchInfo { type patch; }
}
}
}
}
refinementRegions
{
CAD
{
mode inside;
levels ((1E15 2));
}
}
locationInMesh (1e-5 1e-5 1e-5); // Offset from (0 0 0) to avoid
// coinciding with face or edge
}
snapControls
{
// explicitFeatureSnap true;
// implicitFeatureSnap false;
}
addLayersControls
{
layers
{
"CAD.*"
{
nSurfaceLayers 2;
}
}
relativeSizes true; // false, usually with firstLayerThickness
expansionRatio 1.2;
finalLayerThickness 0.5;
minThickness 1e-3;
// firstLayerThickness 0.01;
// maxThicknessToMedialRatio 0.6;
}
meshQualityControls
{
// minTetQuality -1e+30;
}
writeFlags
(
scalarLevels
layerSets
layerFields
);
mergeTolerance 1e-6;
// ************************************************************************* //

35
etc/templates/inflowOutflow/system/surfaceFeatureExtractDict Normal file
View File

@ -0,0 +1,35 @@
/*--------------------------------*- 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 surfaceFeatureExtractDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
CAD.obj
{
extractionMethod extractFromSurface;
extractFromSurfaceCoeffs
{
includedAngle 150;
}
subsetFeatures
{
nonManifoldEdges yes;
openEdges yes;
}
writeObj yes;
}
// ************************************************************************* //