zhyang-dev/OpenFOAM-6
1
0
Fork 0
mirror of https://github.com/OpenFOAM/OpenFOAM-6.git synced 2025-12-08 06:57:46 +00:00
Code Issues Actions Packages Projects Releases Wiki Activity

etc/caseDicts: added useful examples of common dictionary files

Browse Source 
including decomposeParDict, mapFieldsDict, setFieldsDict, surfaceFeaturesDict,
createBafflesDict, createPatchDict, snappyHexMeshDict, extrudeMeshDict and
collapseDict
This commit is contained in:
Chris Greenshields
2018-06-11 12:27:40 +01:00
parent e757494134
commit 3510204297
11 changed files with 660 additions and 0 deletions
Download Patch File Download Diff File Expand all files Collapse all files

62
etc/caseDicts/mesh/generation/collapseDict Normal file
View File

@ -0,0 +1,62 @@
/*--------------------------------*- 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 collapseDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
// If on, adhere to quality criteria in controlMeshQualityCoeffs
controlMeshQuality on;
controlMeshQualityCoeffs
{
#includeEtc "caseDicts/mesh/generation/meshQualityDict"
edgeReductionFactor 0.5;
faceReductionFactor 0.5;
maximumSmoothingIterations 2;
maximumIterations 10;
maxPointErrorCount 5;
}
collapseEdgesCoeffs
{
// Absolute length of edges that are merged
minimumEdgeLength 1e-6;
// The maximum angle between edges that permits merging
maximumMergeAngle 30;
}
collapseFacesCoeffs
{
// The initial face length factor
initialFaceLengthFactor 0.5;
// Relative length of face for collapsing to a point
maxCollapseFaceToPointSideLengthCoeff 0.3;
// Allow early collapse of edges to a point
allowEarlyCollapseToPoint on;
// Factor to premultiply maxCollapseFaceTo... for early collapse
allowEarlyCollapseCoeff 0.2;
// Limiting relative distance between a vertex and face centre
guardFraction 0.1;
}
// ************************************************************************* //

83
etc/caseDicts/mesh/generation/extrudeMeshDict Normal file
View File

@ -0,0 +1,83 @@
/*--------------------------------*- 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 extrudeMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
constructFrom patch;
/*
patch: patch of sourceCase
mesh: patch of sourceCase, retaining original mesh
surface: surface geometry file
*/
sourceCase "$FOAM_CASE"; // uses current case; can be a separate case
sourcePatches (front);
// surface "geometry.obj"; // constructFrom surface
// constructFrom patch: name of exposed "original" patch
exposedPatchName back;
flipNormals false;
extrudeModel plane;
/*
linearNormal: linear extrusion in point-normal direction
plane: single-layer, point-normal extrusion with empty type (2D)
linearDirection: linear extrusion in specified direction
wedge: single-layer, wedge extrusion with wedge type (axisymmetric)
sector: sector extrusion about specified axis
linearRadial: linear extrusion in radial direction
radial: linear extrusion in radial direction with multiple radii
*/
thickness 0.5; // used by plane extrusion
nLayers 10;
expansionRatio 1.0;
// Merge front and back patches, typically for 360 deg wedge extrusion
mergeFaces false;
mergeTol 0;
linearNormalCoeffs
{
thickness 0.5;
}
linearDirectionCoeffs
{
direction (0 1 0);
thickness 0.5;
}
sectorCoeffs // used by sector and wedge extrusion
{
axisPt (0 0 0);
axis (1 0 0);
angle 360;
}
linearRadialCoeffs
{
R 0.5;
Rsurface 0.1;
}
radialCoeffs
{
R table ((0 0.01) (3 0.03) (10 0.1));
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

124
etc/caseDicts/mesh/generation/snappyHexMeshDict Normal file
View File

@ -0,0 +1,124 @@
/*--------------------------------*- 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
{
type triSurfaceMesh;
file "CAD.obj";
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;
inGroups (inlet);
}
}
<outletPatch>
{
level (2 2);
patchInfo
{
type patch;
inGroups (outlet);
}
}
}
}
}
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
nCellsBetweenLevels 3;
}
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;
}
writeFlags
(
// scalarLevels
layerSets
layerFields
);
mergeTolerance 1e-6;
// ************************************************************************* //

46
etc/caseDicts/mesh/manipulation/AMI/createBafflesDict 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 dictionary;
object createBafflesDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
internalFacesOnly true;
baffles
{
baffleFaces
{
type faceZone;
zoneName rotatingZone;
patches
{
master
{
name AMI1;
type cyclicAMI;
matchTolerance 0.0001;
neighbourPatch AMI2;
transform noOrdering;
}
slave
{
$master;
name AMI2;
neighbourPatch AMI1;
}
}
}
}
// ************************************************************************* //

56
etc/caseDicts/mesh/manipulation/AMI/createPatchDict Normal file
View File

@ -0,0 +1,56 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object createPatchDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
pointSync false;
// AMI created from internal boundary with cylinder and cylinder_slave patches
masterAMI
{
name AMI1;
patchInfo
{
type cyclicAMI;
matchTolerance 0.0001;
neighbourPatch AMI2;
transform noOrdering;
}
constructFrom patches;
patches (cylinder);
}
patches
(
// master AMI patch
{
$masterAMI;
}
// slave AMI patch
{
$masterAMI;
name AMI2;
patchInfo
{
neighbourPatch AMI1;
}
patches (cylinder_slave);
}
);
// ************************************************************************* //

47
etc/caseDicts/mesh/manipulation/baffles/createBafflesDict 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 dictionary;
object createBafflesDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
// Whether to convert internal faces only (so leave boundary faces intact).
// This is only relevant if your face selection type can pick up boundary
// faces.
internalFacesOnly true;
// Example using "blades" as name of baffle patch
baffles
{
baffles // group name
{
//- Use predefined faceZone to select faces and orientation.
type faceZone;
zoneName blades;
patches
{
master
{
name blades; // patch name
type wall;
}
slave
{
$master;
}
}
}
}
// ************************************************************************* //

42
etc/caseDicts/mesh/manipulation/patches/createPatchDict 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;
object createPatchDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
pointSync false;
patches
(
{
name inlet;
patchInfo
{
type patch;
}
constructFrom set;
set inletFaces;
}
{
name walls;
patchInfo
{
type wall;
}
constructFrom patches;
patches ("CAD.*");
}
);
// ************************************************************************* //

41
etc/caseDicts/preProcessing/decomposeParDict Normal file
View File

@ -0,0 +1,41 @@
/*--------------------------------*- 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 decomposeParDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
numberOfSubdomains 8;
/*
Main methods are:
1) Geometric: "simple"; "hierarchical", with ordered sorting, e.g. xyz, yxz
2) Scotch: "scotch", when running in serial; "ptscotch", running in parallel
*/
method hierarchical;
simpleCoeffs
{
n (4 2 1); // total must match numberOfSubdomains
delta 0.001;
}
hierarchicalCoeffs
{
n (4 2 1); // total must match numberOfSubdomains
delta 0.001;
order xyz;
}
// ************************************************************************* //

31
etc/caseDicts/preProcessing/mapFieldsDict Normal file
View File

@ -0,0 +1,31 @@
/*--------------------------------*- 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 mapFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
// Map data from source patch to target coincident patch
patchMap
(
<sourcePatch1> <targetPatch1>
<sourcePatch2> <targetPatch2>
);
// Target patches whose field values are mapped from the internal source mesh
cuttingPatches
(
<targetPatch1>
<targetPatch2>
);
// ************************************************************************* //

67
etc/caseDicts/preProcessing/setFieldsDict 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 setFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
defaultFieldValues
(
volScalarFieldValue alpha.water 0
volVectorFieldValue U (0 0 0)
);
regions
(
// Setting values inside a box
boxToCell
{
box (0 0 0) (30 30 30);
fieldValues
(
volScalarFieldValue alpha.water 1
volVectorFieldValue U (1 0 0)
);
}
// Setting values inside a sphere
sphereToCell
{
centre (40 40 40);
radius 10;
fieldValues
(
volScalarFieldValue alpha.water 1
volVectorFieldValue U (1 0 0)
);
}
// Setting values inside a surface geometry file
surfaceToCell
{
file "geometry.obj";
outsidePoints ( (0 0 0) );
includeCut no;
includeInside yes;
includeOutside no;
nearDistance 0;
curvature 0;
fieldValues
(
volScalarFieldValue alpha.water 1
volVectorFieldValue U (1 0 0)
);
}
);
// ************************************************************************* //

61
etc/caseDicts/surface/surfaceFeaturesDict Normal file
View File

@ -0,0 +1,61 @@
/*--------------------------------*- 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;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
surfaces
(
"surface1.stl"
"surface2.obj"
);
// Identify edges when angle between faces < includedAngle
includedAngle 120;
// Include region boundaries as features
geometricTestOnly no;
subsetFeatures
{
// Include only edges that intersect the plane with (normal)(basePoint)
// plane (1 0 0)(0 0 0);
// Include only edges inside the box
// insideBox (0 0 0)(1 1 1);
// Include only edges outside the box
// outsideBox (0 0 0)(1 1 1);
// Include nonManifold edges (edges with >2 connected faces)
nonManifoldEdges yes;
// Include open edges (edges with 1 connected face)
openEdges yes;
}
trimFeatures
{
// Remove features with fewer than the specified number of edges
minElem 0;
// Remove features shorter than the specified cumulative length
minLen 0.0;
}
// Write features to obj format for visualisation
writeObj yes;
verboseObj no;
// ************************************************************************* //