The legacy fvMeshTopoChangersMovingCone removed, replaced by the more general
mesh mapping approach, see tutorials incompressibleFluid/movingCone and
shockFluid/movingCone.
A number of fixes have been made in order to make non-conformal cyclic
patches compatible with run-time distribution.
A tutorial case, incompressibleVoF/rotatingCube, has been added which
demonstrates simultaneous usage of motion, non-conformal couplings,
adaptive refinement and load-balancing.
Now both the checkMesh utility and functionObject operate in the same manner
with the same controls, executing the same checkGeometry and checkTopology
functions from the new meshCheck library. The controls have been updated and
made more consistent and flexible, in particular by the addition of optional
user specification for the non-orthogonality and skewness error thresholds:
Application
checkMesh
Description
Checks validity of a mesh.
Usage
\b checkMesh [OPTION]
Options:
- \par noTopology
Skip checking the mesh topology
- \par -allTopology
Check all (including non finite-volume specific) addressing
- \par -allGeometry
Check all (including non finite-volume specific) geometry
- \par -meshQuality
Check against user defined (in \a system/meshQualityDict) quality
settings
- \par -region \<name\>
Specify an alternative mesh region.
- \par -writeSurfaces
Reconstruct cellSets and faceSets of problem faces and write to
postProcessing directory.
- \par -surfaceFormat <format>
Format used to write the cellSets and faceSets surfaces
e.g. vtk or ensight.
- \par -writeSets
Reconstruct pointSets of problem points nd write to
postProcessing directory.
- \par -setFormat <format>
Format used to write the pointSets
e.g. vtk or ensight.
- \par -nonOrthThreshold <threshold value in degrees>
Threshold in degrees for reporting non-orthogonality errors,
default: 70"
- \par -skewThreshold <threshold value>
Threshold for reporting skewness errors, default: 4.
Class
Foam::functionObjects::checkMesh
Description
Executes primitiveMesh::checkMesh(true) every execute time for which the
mesh changed, i.e. moved or changed topology.
Useful to check the correctness of changing and morphing meshes.
Usage
\table
Property | Description | Required | Default value
type | type name: checkMesh | yes |
noTopology | Skip checking the mesh topology | no | false
allTopology | Check all addressing | no | false
allGeometry | Check all geometry | no | false
writeSurfaces | Reconstruct and write problem faces | no | false
surfaceFormat | Format for problem faceSets | no | vtk
writeSets | Reconstruct and write problem points | no | false
setFormat | Format used to write the problem pointSets | no | vtk
nonOrthThreshold | Threshold for non-orthogonality errors | no | 70 deg
skewThreshold | Threshold for reporting skewness errors | no | 4
\endtable
Example of checkMesh specification:
\verbatim
checkMesh
{
type checkMesh;
libs ("libutilityFunctionObjects.so");
executeControl timeStep;
executeInterval 10;
allGeometry true;
allTopology true;
writeSurfaces true;
surfaceFormat vtk;
writeSets true;
setFormat vtk;
}
\endverbatim
or using the standard configuration file:
\verbatim
#includeFunc checkMesh(executeInterval=10, allGeometry=true)
\endverbatim
This avoids potential hidden run-time errors caused by solvers running with
boundary conditions which are not fully specified. Note that "null-constructor"
here means the constructor from patch and internal field only, no data is
provided.
Constraint and simple BCs such as 'calculated', 'zeroGradient' and others which
do not require user input to fully specify their operation remain on the
null-constructor table for the construction of fields with for example all
'calculated' or all 'zeroGradient' BCs.
A special version of the 'inletOutlet' fvPatchField named 'zeroInletOutlet' has
been added in which the inlet value is hard-coded to zero which allows this BC
to be included on the null-constructor table. This is useful for the 'age'
functionObject to avoid the need to provide the 'age' volScalarField at time 0
unless special inlet or outlet BCs are required. Also for isothermalFilm in
which the 'alpha' field is created automatically from the 'delta' field if it is
not present and can inherit 'zeroInletOutlet' from 'delta' if appropriate. If a
specific 'inletValue' is require or other more complex BCs then the 'alpha'
field file must be provided to specify these BCs as before.
Following this improvement it will now be possible to remove the
null-constructors from all fvPatchFields not added to the null-constructor
table, which is most of them, thus reducing the amount of code and maintenance
overhead and making easier and more obvious to write new fvPatchField types.
This completes commit 381e0921 and permits patches on the "top" of
extruded regions to determine the point locations opposite as well as
the face centres and areas. This means that patches with dissimilar
meshes can now be coupled via the patchToPatch interpolation engine.
A few fixes have also been applied to extrudeToRegionMesh to make the
intrude option compatibile with extrusion into internal faces and
between opposing zones/sets/patches. The 'shadow' entries used for
extrusion inbetween opposing zones/sets/patches have also been renamed
to 'opposite' for consistency with the patch names and patch types
entries; e.g.,
faceZones (fz1 fz3);
oppositeFaceZones (fz2 fz4); // <-- was 'faceZonesShadow'
faceSets (fs1 fs3);
oppositeFaceSets (fs2 fs4); // <-- was 'faceSetsShadow'
patches (p1 p3);
oppositePatches (p2 p4); // <-- was 'patchesShadow'
With the new film implementation the single cell layer film region is extruded
into (overlapping with) the primary/fluid region which can now be generated with
extrudeToRegionMesh using the new 'intrude' option, e.g. for the
tutorials/modules/multiRegion/film/splashPanel case the extrudeToRegionMeshDict
contains:
region film;
patches (film);
extrudeModel linearNormal;
intrude yes;
adaptMesh no;
patchTypes (mappedExtrudedWall);
patchNames (film);
regionPatchTypes (filmWall);
regionPatchNames (wall);
regionOppositePatchTypes (mappedFilmSurface);
regionOppositePatchNames (surface);
nLayers 1;
expansionRatio 1;
linearNormalCoeffs
{
thickness 0.002;
}
genericPatches is linked into mesh generation and manipulation utilities but not
solvers so that the solvers now check for the availability of the specified
patch types. Bugs in the tutorials exposed by this check have been corrected.
e.g. in extrudeToRegionMeshDict:
// Generate the region named film
region film;
// from the patch extrudeWall
patches (extrudeWall);
// generating mapped patches for the extruded region
adaptMesh yes;
// New options:
// Set the type of the mapped patch on the existing mesh to mappedWall ...
patchTypes (mappedWall);
// ... and name to wall
patchNames (wall);
// Set the type of the mapped patch on the region mesh to mappedFilmWall ...
regionPatchTypes (mappedFilmWall);
// ... and name to wall
regionPatchNames (wall);
// Set the type of the opposite patch on the region mesh to empty ...
regionOppositePatchTypes (empty);
// ... and name to empty
regionOppositePatchNames (empty);
All the above entries are optional and if not present the previous behaviour is
reproduced.
Replaces MeshObject, providing a formalised method for creating demand-driven
mesh objects, optionally supporting update functions called by the mesh
following mesh changes.
Class
Foam::DemandDrivenMeshObject
Description
Templated abstract base-class for demand-driven mesh objects used to
automate their allocation to the mesh database and the mesh-modifier
event-loop.
DemandDrivenMeshObject is templated on the type of mesh it is allocated
to, the type of the mesh object (TopologicalMeshObject, GeometricMeshObject,
MoveableMeshObject, DistributeableMeshObject, UpdateableMeshObject) and the
type of the actual object it is created for example:
\verbatim
class leastSquaresVectors
:
public DemandDrivenMeshObject
<
fvMesh,
MoveableMeshObject,
leastSquaresVectors
>
{
.
.
.
//- Delete the least square vectors when the mesh moves
virtual bool movePoints();
};
\endverbatim
MeshObject types:
- TopologicalMeshObject: mesh object to be deleted on topology change
- GeometricMeshObject: mesh object to be deleted on geometry change
- MoveableMeshObject: mesh object to be updated in movePoints
- UpdateableMeshObject: mesh object to be updated in topoChange or
movePoints
- PatchMeshObject: mesh object to be additionally updated patch changes
DemandDrivenMeshObject should always be constructed and accessed via the New
methods provided so that they are held and maintained by the objectRegistry.
To ensure this use constructors of the concrete derived types should be
private or protected and friendship with the DemandDrivenMeshObject
base-class declared so that the New functions can call the the constructors.
Additionally the mesh-object types (TopologicalMeshObject, GeometricMeshObject,
MoveableMeshObject, DistributeableMeshObject, UpdateableMeshObject) can now be
used as mix-in types for normally allocated objects providing the same interface
to mesh-change update functions, see the Fickian fluid
thermophysicalTransportModel or anisotropic solid thermophysicalTransportModel.
This new approach to adding mesh-update functions to classes will be applied to
other existing classes and future developments to simplify the support and
maintenance of run-time mesh changes, in particular mesh refinement/unrefinement
and mesh-to-mesh mapping.
The timeName() function simply returns the dimensionedScalar::name() which holds
the user-time name of the current time and now that timeName() is no longer
virtual the dimensionedScalar::name() can be called directly. The timeName()
function implementation is maintained for backward-compatibility.
A set of routines for cutting polyhedra have been added. These can cut
polyhedral cells based on the adjacent point values and an iso-value
which defines the surface. The method operates directly on the
polyhedral cells; it does not decompose them into tetrahedra at any
point. The routines can compute the cut topology as well as integrals of
properties above and below the cut surface.
An iso-surface algorithm has been added based on these polyhedral
cutting routines. It is significantly more robust than the previous
algorithm, and produces compact surfaces equivalent to the previous
algorithm's maximum filtering level. It is also approximately 3 times
faster than the previous algorithm, and 10 times faster when run
repeatedly on the same set of cells (this is because some addressing is
cached and reused).
This algorithm is used by the 'isoSurface', 'distanceSurface' and
'cutPlane' sampled surfaces.
The 'cutPlane' sampled surface is a renaming of 'cuttingPlane' to make
it consistent with the corresponding packaged function. The name
'cuttingPlane' has been retained for backwards compatibility and can
still be used to select a 'cutPlane' surface. The legacy 'plane' surface
has been removed.
The 'average' keyword has been removed from specification of these
sampled surfaces as cell-centred values are no longer used in the
generation of or interpolation to an iso-surface. The 'filtering'
keyword has also been removed as it relates to options within the
previous algorithm. Zone support has been reinstated into the
'isoSurface' sampled surface. Interpolation to all these sampled
surfaces has been corrected to exactly match the user-selected
interpolation scheme, and the interpolation procedure no longer
unnecessarily re-generates data that is already available.
If checkMesh is executed with the -allGeometry option, then surface
files containing the NCC coverage will now be written out. Coverage is
the ratio between coupled area magnitude and total area magnitude. This
is useful for locating parts of the boundary mesh that are in error.
Errors (such as folds and pinches) typically manifest as a coverage
value that deviates significantly from a value of one.
This is comparable to the writing of AMI patches's weight sums, which
also used to occur when the -allGeometry option was selected.
