songtianlun/openfoam
1
0
Fork 0
Code Issues Pull Requests Actions Packages Projects Releases Wiki Activity

ENH: refineMesh: tutorial to demo directional refinement

Browse Source
This commit is contained in:
mattijs 2025-01-27 17:24:35 +00:00
parent 6dc57a1a8b
commit 0b831572f3
11 changed files with 477 additions and 0 deletions
Show Stats Download Patch File Download Diff File Expand all files Collapse all files

10
tutorials/mesh/refineMesh/cylinder/Allclean Executable file
View File

@ -0,0 +1,10 @@
#!/bin/sh
cd "${0%/*}" || exit # Run from this directory
. ${WM_PROJECT_DIR:?}/bin/tools/CleanFunctions # Tutorial clean functions
#------------------------------------------------------------------------------
cleanCase
rm -rf constant
#------------------------------------------------------------------------------

26
tutorials/mesh/refineMesh/cylinder/Allrun Executable file
View File

@ -0,0 +1,26 @@
#!/bin/sh
cd "${0%/*}" || exit # Run from this directory
. ${WM_PROJECT_DIR:?}/bin/tools/RunFunctions # Tutorial run functions
#------------------------------------------------------------------------------
mkdir -p constant/triSurface
cp -f \
"$FOAM_TUTORIALS"/resources/geometry/cylinder.vtk.gz \
constant/triSurface/
# Generate mesh from surface (in constant/triSurface)
runApplication extrudeMesh
# Make front and back type empty
runApplication createPatch -overwrite
runApplication -s "level1" topoSet -dict system/topoSetDict_level1
runApplication -s "level1" refineMesh
runApplication -s "level2" topoSet -dict system/topoSetDict_level2
runApplication -s "level2" refineMesh
#------------------------------------------------------------------------------

1
tutorials/mesh/refineMesh/cylinder/README.txt Normal file
View File

@ -0,0 +1 @@
Demonstrate using user-defined coordinate system to directionally refine.

48
tutorials/mesh/refineMesh/cylinder/system/controlDict Normal file
View File

@ -0,0 +1,48 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2412 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application snappyHexMesh;
startFrom latestTime;
startTime 0;
stopAt endTime;
endTime 100;
deltaT 1;
writeControl runTime;
writeInterval 1;
purgeWrite 0;
writeFormat ascii;
writePrecision 6;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable true;
// ************************************************************************* //

84
tutorials/mesh/refineMesh/cylinder/system/createPatchDict Normal file
View File

@ -0,0 +1,84 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2412 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object createPatchDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
pointSync false;
// Patches to create.
patches
(
{
// Name of new patch
name oversetPatch;
// Dictionary to construct new patch from
patchInfo
{
type overset;
}
// How to construct: either from 'patches' or 'set'
constructFrom patches;
// If constructFrom = patches : names of patches. Wildcards allowed.
patches (otherSide);
// If constructFrom = set : name of faceSet
set f0;
}
{
// Name of new patch
name walls;
// Dictionary to construct new patch from
patchInfo
{
type wall;
}
// How to construct: either from 'patches' or 'set'
constructFrom patches;
// If constructFrom = patches : names of patches. Wildcards allowed.
patches (originalPatch);
// If constructFrom = set : name of faceSet
set f0;
}
{
// Name of new patch
name frontAndBack;
// Dictionary to construct new patch from
patchInfo
{
type empty;
}
// How to construct: either from 'patches' or 'set'
constructFrom patches;
// If constructFrom = patches : names of patches. Wildcards allowed.
patches (sides);
// If constructFrom = set : name of faceSet
set f0;
}
);
// ************************************************************************* //

135
tutorials/mesh/refineMesh/cylinder/system/extrudeMeshDict Normal file
View File

@ -0,0 +1,135 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2412 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object extrudeMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
// What to extrude:
// patch : from patch of another case ('sourceCase')
// mesh : as above but with original case included
// surface : from externally read surface
//constructFrom mesh;
//constructFrom patch;
constructFrom surface;
// If construct from patch/mesh:
sourceCase "../cavity";
sourcePatches (movingWall);
// If construct from patch: patch to use for back (can be same as sourcePatch)
exposedPatchName movingWall;
// If construct from surface:
surface "<constant>/triSurface/cylinder.vtk";
// Flip surface normals before usage. Valid only for extrude from surface or
// patch.
flipNormals false;
//- Linear extrusion in point-normal direction
extrudeModel linearNormal;
//- Single layer linear extrusion in point-normal direction
// with empty patches on front and back
//extrudeModel plane;
//- Linear extrusion in specified direction
//extrudeModel linearDirection;
//- Sector extrusion
//extrudeModel sector;
//- Wedge extrusion of a single layer
// with wedge patches on front and back
//extrudeModel wedge;
//- Extrudes into sphere around (0 0 0)
//extrudeModel linearRadial;
//- Extrudes into sphere around (0 0 0) with specified radii
//extrudeModel radial;
//- Extrudes into sphere with grading according to pressure (atmospherics)
//extrudeModel sigmaRadial;
//- Extrudes by interpolating along path inbetween two (topologically identical)
// surfaces (e.g. one is an offsetted version of the other)
//extrudeModel offsetSurface;
nLayers 10;
expansionRatio 1.02;
sectorCoeffs //<- Also used for wedge
{
point (0 0.1 -0.05);
axis (-1 0 0);
angle 360; // For nLayers=1 assume symmetry so angle/2 on each side
}
linearNormalCoeffs
{
thickness 0.7;
}
planeCoeffs
{
// thickness 0.1;
nLayers 4;
}
linearDirectionCoeffs
{
direction (0 1 0);
thickness 0.5;
}
linearRadialCoeffs
{
R 0.1;
Rsurface 0.01; // Optional inner radius
}
radialCoeffs
{
// Radii specified through interpolation table
R table ((0 0.01)(3 0.03)(10 0.1));
}
sigmaRadialCoeffs
{
RTbyg 1;
pRef 1;
pStrat 1;
}
offsetSurfaceCoeffs
{
// Surface that mesh has been meshed to
baseSurface "<constant>/triSurface/DTC-scaled-inflated.obj";
// Surface to fill in to
offsetSurface "<constant>/triSurface/DTC-scaled.obj";
}
// Do front and back need to be merged? Usually only makes sense for 360
// degree wedges.
mergeFaces false;
// Merge small edges. Fraction of bounding box.
mergeTol 0;
// ************************************************************************* //

42
tutorials/mesh/refineMesh/cylinder/system/fvSchemes Normal file
View File

@ -0,0 +1,42 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2412 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
}
gradSchemes
{
}
divSchemes
{
}
laplacianSchemes
{
}
interpolationSchemes
{
}
snGradSchemes
{
}
// ************************************************************************* //

23
tutorials/mesh/refineMesh/cylinder/system/fvSolution Normal file
View File

@ -0,0 +1,23 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2412 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
PIMPLE
{
nOuterCorrectors 1;
}
// ************************************************************************* //

42
tutorials/mesh/refineMesh/cylinder/system/refineMeshDict Normal file
View File

@ -0,0 +1,42 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2406 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object refineMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
set cellsToRefine;
coordinateSystem user;
userCoeffs
{
type cylindrical;
origin (0 0 0);
e1 (1 0 0);
e3 (0 1 0);
}
directions
(
//normal
tan1
//tan2
);
useHexTopology true;
geometricCut false;
writeMesh false;
// ************************************************************************* //

33
tutorials/mesh/refineMesh/cylinder/system/topoSetDict_level1 Normal file
View File

@ -0,0 +1,33 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2406 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name cellsToRefine;
type cellSet;
action new;
// Mandatory entries
source cylinderAnnulusToCell;
p1 (0 -1 0);
p2 (0 1 0);
innerRadius 0.7;
outerRadius 1.5;
}
);
// ************************************************************************* //

33
tutorials/mesh/refineMesh/cylinder/system/topoSetDict_level2 Normal file
View File

@ -0,0 +1,33 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2406 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
{
name cellsToRefine;
type cellSet;
action new;
// Mandatory entries
source cylinderAnnulusToCell;
p1 (0 -1 0);
p2 (0 1 0);
innerRadius 0.9;
outerRadius 1.5;
}
);
// ************************************************************************* //