OpenFOAM中原生网格生成方法与操作组件介绍
2014-05-30 21:42阅读：
Notes for Native Mesh Method in OpenFOAM
★The OpenFOAM tutorials and CFD-online forum are
the two most useful tools!
1. blockMesh
Keyword: structure mesh(Hex), base grids
for snappyHexMesh
Execute:
blockMesh
Requirements:
Dictionary file
constant/polyMesh/blockMeshDict
Dictionary system/controlDict
blockMeshDict:
convertToMeters : used for unit conversion,
default unit in OF is m(SI). (it seems no use)
vertices: define points of the domain in 3D format, and
number them from 0 (feature in C++).
blocks: define blocks (list of vertices must start from
the face with minX and then to the face with maxX when use as
the base mesh for snappyHexMesh)
.
edges: use to describe arc or spline edges
(U-139).
boundary : define and name the faces which could
be used later as boundaries.
mergePatchPairs: list of patches to be merged and can be
omitted.
Fig 1 a simple hex block
|
Notes: blockMesh can be used to
generate structured mesh, but it could be very complicated to
manipulate for 3 dimensional model and other complex geometries the
curves and surfaces. However it is essential to use
blockMesh to generate the base mesh for
snappyHexMesh.
Example:
convertToMeters 1;
vertices
(
(-15000 -10000 -10000)
//
0
(-15000 20000 -10000)
// 1
(15000 20000 -10000)
// 2
(15000 -10000 -10000)
// 3
(-15000 -10000 10000)
// 4
(-15000 20000 10000)
// 5
(15000 20000 10000)
// 6
(15000 -10000 10000)
// 7
);
blocks
(
//hex (0 1 2 3 4 5 6 7) (25 20 20)
simpleGrading (1 1 1)
hex (0 1 5 4 3 2 6 7) (25 20 20)
simpleGrading (1 1 1)
// hex must starts with the
face at minX then the face at maxX(or from maxX to
minX)
// ! Otherwise, it will go wrong
when doing snappyHexMesh
);
edges
// Ref
U-139
(
);
boundary
(
frontAndBack
{
type patch;
faces
(
(3 7 6 2)
(1 5 4 0)
);
}
inlet
{
type patch;
faces
(
(0 4 7 3)
);
}
outlet
{
type patch;
faces
(
(2 6 5 1)
);
}
lowerWall
{
type wall;
faces
(
(0 3 2 1)
);
}
upperWall
{
type patch;
faces
(
(4 5 6 7)
);
}
);
2. snappyHexMesh
Keywords: hex-dominate mesh, cut-cell,
complex (or called arbitrary) geometry
Execute: snappyHexMesh
[-overwrite]
Requirements:
Essential:
system/snappyHexMeshDict
the control file for this
utility
constant/triSurface/
the geometry of the target, can be in the
format of stl, obj or nas.
Optional:
systemt/surfaceFeatureExtractDict
the control file for surface feature extract. In
order to capture the features of a geometry with complicated
surfaces, users should extract these features by run the utility
called surfaceFeatureExtract before
snappyHexMesh. During the extraction, a series of
files will be generated in directory
constant/extendedFeatureEdgeMesh.
system/decomposeParDict
control
file for snappyHexMesh in parallel.
system/meshQualityDict
control file could be included in file
snappyHexMeshDict.
Advantages:Being native in OpenFoam,
snappyHexMesh is fully compatible with parallel
process, zonal meshing for MRF and boundary layers.
Steps:
a)
Creat the base mesh with
blockMesh.
b)
Check the domain and boundaries in
ParaView and prepare the refine zone(refinement box etc.).
Open both of the geometry(*.stl etc.) and the base
mesh.
c)
(optional) Run
surfaceFeatureExtract to generate all the needed
features of your geometry.
d)
Define the parameters in snappyHexMeshDict including
geometry, refinementBox, feature, refinementSurfaces,
refinementRigion, locationInMesh, layers etc.
e)
(optional) Run
decomposePar to get the processors’
directories.
f)
Run snappyHexMesh or
mpirun -np 4 snappyHexMesh -overwrite –parallel to
generate grids.
g)
(optional) reconstructParMesh
–constant.
Notes:
l
snappyHexMeshDict (geometry +
castellatedMeshControls + snapControls + addLayersControls +
meshQualityControls)
l
Be careful with all the geometry names
use in files, even the name exist in the file header of
*.stl.
Example:
The helicopter called SA342 includes complicated surfaces and
gaps, and this problem also belong to the external aerodynamic.
Therefore, the SA342 was chosen as the geometry in this
section.
Fig 2 snappyHexMesh for SA342
helicopter
The easiest way to set up your case is copy a similar
tutorial into your working directory and then change some specified
parameters to yours. As a kind of incompressible external flow at
low Reynolds number, the tutorial called motorBike in
OpenFOAM became the templates. Some important codes with comments
were listed in the following.
surfaceFeatureExtractDict
SA342.stl
{
// How to obtain raw features
(extractFromFile || extractFromSurface)
extractionMethod
extractFromSurface;
extractFromSurfaceCoeffs
{
//
Mark edges whose adjacent surface normals are at an angle
less
//
than includedAngle as features
//
- 0 : selects no edges
//
- 180: selects all edges
includedAngle 150;
}
subsetFeatures
{
//
Keep nonManifold edges (edges with >2 connected
faces)
nonManifoldEdges
no;
//
Keep open edges (edges with 1 connected face)
openEdges
yes;
}
// Write options
//
Write features to obj format for postprocessing
writeObj
yes;
}
surfaceFeatureExtractDict is often
been kept as default except for the includedAngle in
extractFromSurfaceCoeffs.
snappyHexMeshDict:
geometry
// define the geometry in your project
{
SA342.stl
// the
geometry file’s name in constant/triSurface
{
type triSurfaceMesh;
name SA342;
// give a name to your geometry
which will be used later.
}
refinementBox
// zone of refinement, could be Box,
Sphere, and cylinder
{
type searchableBox;
min (-4000 -1500 -1000);
max ( 4000 8000 5000);
}
// this zone could also be
visualized and checked in ParaView
};
//
features
(
{
file 'SA342.eMesh';
// *.eMesh file is generated by
surfaceFeatureExtract
level 6;
}
);
//
refinementSurfaces
{
SA342
{
// Surface-wise min and max
refinement level
level (5 6);
// Optional specification of patch
type (default is wall). No
// constraint types (cyclic,
symmetry) etc. are allowed.
patchInfo
{
type wall;
inGroups (SA342); // this name
should be the same with that in your *.stl file
}
}
//
refinementRegions
{
refinementBox
{
mode inside;
// select the
region which will be refined
levels ((1E15 4));
}
}
locationInMesh (0.05 6000.05 2000.05);
// This point should better to be
in this style rather than only integer
//
layers
{
'SA342'
{
nSurfaceLayers 1;
// the
number of layers
}
}
// Expansion factor for layer
mesh
expansionRatio
1.0;
3. Other utilities for mesh maniputation
1.
autoPatch
Execution: autoPatch [-overwrite]
Identify different patches by featured angle.
2.
checkMesh
Keywords: mesh quality and write
different zones into set directory
Execution: checkMesh [–allGeometry] [–allTopology]
[–constant] [-noZero]
Requirements
mesh file in constant/polyMesh
Dictionary system/controlDict
The utility will check whether your mesh can be calculated by
OpenFOAM and report the quality of you mesh. In addition, users can
get some summary information form the check report.
In addition, after executing this utility, different zones
will be distinguished and the results will exist in the
directory constant/polyMesh/sets.
3.
createPatch
Keywords: create / modify
patches
Execution: createPatch [–dict]
[–overwrite]
Requirements
Dictionary system/createPatchDict
// Patches to create.
patches
(
{
name inlet;
patchInfo
{
type
patch;
}
constructFrom set;
set inletFaces;
}
);
4.
decomposePar /
recomposeParMesh
Keywords: parallel
Only used in parallel calculation.
5.
extrudeMesh
Keywords: 2D/3D mesh
Execution: extrudeMesh
[-overwrite]
Requirements:extrudeMeshDict
This utility extrudes 2D mesh (or patch) into 3D mesh, or can
be used to generate a OpenFOAM 2D mesh by extruding a patch by one
element in z direction. Results will be saved in a new time
sequence file.
extrudeMeshDict:
constructFrom patch;
// indicate the source to be extrude is
patch
sourceCase '../rotor';
//
source case directory
sourcePatches (auto2);
// source
patch name
extrudeModel
linearNormal;
// model: linearNormal or
wedge
nLayers
50;
expansionRatio
1.0;
linearNormalCoeffs
{
thickness
1.21;
// thickness
}
6.
mergeMeshes
Keywords:hybrid mesh
Execution: mergeMeshes masterDir
addDir [-overwrite]
This utility can be used to merge different meshes in to one.
And its most important use may be to generate a hybrid
mesh.
7.
patchSummary
This is useful to check your patches or
boundaries.
8.
renumberMesh
Execution:
renumberMesh
This utility is used for renumbering the mesh and reducing
the bandwidth of the unstructured grids(CM method), which could
improve the efficiency of iteration.
9.
transformPoints
Keywords:scale, translate,
rotate
Execution: transformPoints –translate ‘(0 0
0.1)’
10.
topoSet
Keywords:topology, zones
Execution: topoSet
Requirements:topSetDict
Set up basic topology with specified rules, including
geometry and patches.
topoSetDict:
actions
(
{
name
rotor;
type
cellSet;
// type:
cellSet => constant/polyMesh/cellZones
action
new;
source cylinderToCell;
// more
types on google
sourceInfo
{
p1 (0.121 0.0
0.00684432); // start point on cylinder
axis//
p2 (0.121 0.0
-0.174509); // end point on cylinder
axis//
radius
0.242;
}
}
{
name
interAMI;
type
faceSet;
action
new;
source
patchToFace;
sourceInfo
{
//
name 'inter.*';
}
}
// write the rotor set to constant/polyMehs/cellZones
file
// rotor
{
name rotor;
type cellZoneSet;
action new;
source setToCellZone;
sourceInfo
{
set
rotor;
}
}
);
11.
potentialFoam
Keywords:potential flow,
initialization
Execution: potentialFoam
–noFunctionObjects –writep
Requirements:fvSolution
Initialize the flow field by solving the potential
equation(Laplacian).
fvSolution:
potentialFlow
{
nNonOrthogonalCorrectors
10;
// number of
iteration
pRefCell
0;
pRefValue
0;
}
注：在OpenFOAM网格学习中整理的笔记，个人理解可能不全面甚至是有错误，本着交流的心态拿出来与大家共享（软件版本OpenFOAM-2.3.x）。
