DecomposePar and reconstructPar now interleave the processing of
multiple regions. This means that with the -allRegions option, the
earlier times are completed in their entirety before later times are
considered. It also lets regions to access each other during
decomposition and reconstruction, which will be important for
non-conformal region interfaces.
To aid interpretation of the log, region prefixing is now used by both
utilities in the same way as is done by foamMultiRun.
DecomposePar has been overhauled so that it matches reconstructPar much
more closely, both in terms of output and of iteration sequence. All
meshes and addressing are loaded simultaneously and each field is
considered in turn. Previously, all the fields were loaded, and each
process and addressing set was considered in turn. This new strategy
optimises memory usage for cases with lots of fields.
The patch field 'autoMap' and 'rmap' functions have been replaced with a
single 'map' function that can used to do any form of in-place
patch-to-patch mapping. The exact form of mapping is now controlled
entirely by the mapper object.
An example 'map' function is shown below:
void nutkRoughWallFunctionFvPatchScalarField::map
(
const fvPatchScalarField& ptf,
const fvPatchFieldMapper& mapper
)
{
nutkWallFunctionFvPatchScalarField::map(ptf, mapper);
const nutkRoughWallFunctionFvPatchScalarField& nrwfpsf =
refCast<const nutkRoughWallFunctionFvPatchScalarField>(ptf);
mapper(Ks_, nrwfpsf.Ks_);
mapper(Cs_, nrwfpsf.Cs_);
}
This single function replaces these two previous functions:
void nutkRoughWallFunctionFvPatchScalarField::autoMap
(
const fvPatchFieldMapper& m
)
{
nutkWallFunctionFvPatchScalarField::autoMap(m);
m(Ks_, Ks_);
m(Cs_, Cs_);
}
void nutkRoughWallFunctionFvPatchScalarField::rmap
(
const fvPatchScalarField& ptf,
const labelList& addr
)
{
nutkWallFunctionFvPatchScalarField::rmap(ptf, addr);
const nutkRoughWallFunctionFvPatchScalarField& nrwfpsf =
refCast<const nutkRoughWallFunctionFvPatchScalarField>(ptf);
Ks_.rmap(nrwfpsf.Ks_, addr);
Cs_.rmap(nrwfpsf.Cs_, addr);
}
Calls to 'autoMap' should be replaced with calls to 'map' with the same
mapper object and the patch field itself provided as the source. Calls
to 'rmap' should be replaced with calls to 'map' by wrapping the
addressing in a 'reverseFvPatchFieldMapper' (or
'reversePointPatchFieldMapper') object.
This change simplifies the creation of new patch fields and hence
improves extensibility. It also provides more options regarding general
mapping strategies between patches. Previously, general abstracted
mapping was only possible in 'autoMap'; i.e., from a patch to itself.
Now, general mapping is possible between different patches.
The reconstructPar utility now reconstructs the mesh if and when it is
necessary to do so. The reconstructParMesh utility is therefore no
longer necessary and has been removed.
It was necessary/advantagous to consolidate these utilities into one
because in the case of mesh changes it becomes increasingly less clear
which of the separate utilities is responsible for reconstructing data
that is neither clearly physical field nor mesh topology; e.g., moving
points, sets, refinement data, and so on.
This major development provides coupling of patches which are
non-conformal, i.e. where the faces of one patch do not match the faces
of the other. The coupling is fully conservative and second order
accurate in space, unlike the Arbitrary Mesh Interface (AMI) and
associated ACMI and Repeat AMI methods which NCC replaces.
Description:
A non-conformal couple is a connection between a pair of boundary
patches formed by projecting one patch onto the other in a way that
fills the space between them. The intersection between the projected
surface and patch forms new faces that are incorporated into the finite
volume mesh. These new faces are created identically on both sides of
the couple, and therefore become equivalent to internal faces within the
mesh. The affected cells remain closed, meaning that the area vectors
sum to zero for all the faces of each cell. Consequently, the main
benefits of the finite volume method, i.e. conservation and accuracy,
are not undermined by the coupling.
A couple connects parts of mesh that are otherwise disconnected and can
be used in the following ways:
+ to simulate rotating geometries, e.g. a propeller or stirrer, in which
a part of the mesh rotates with the geometry and connects to a
surrounding mesh which is not moving;
+ to connect meshes that are generated separately, which do not conform
at their boundaries;
+ to connect patches which only partially overlap, in which the
non-overlapped section forms another boundary, e.g. a wall;
+ to simulate a case with a geometry which is periodically repeating by
creating multiple couples with different transformations between
patches.
The capability for simulating partial overlaps replaces the ACMI
functionality, currently provided by the 'cyclicACMI' patch type, and
which is unreliable unless the couple is perfectly flat. The capability
for simulating periodically repeating geometry replaces the Repeat AMI
functionality currently provided by the 'cyclicRepeatAMI' patch type.
Usage:
The process of meshing for NCC is very similar to existing processes for
meshing for AMI. Typically, a mesh is generated with an identifiable set
of internal faces which coincide with the surface through which the mesh
will be coupled. These faces are then duplicated by running the
'createBaffles' utility to create two boundary patches. The points are
then split using 'splitBaffles' in order to permit independent motion of
the patches.
In AMI, these patches are assigned the 'cyclicAMI' patch type, which
couples them using AMI interpolation methods.
With NCC, the patches remain non-coupled, e.g. a 'wall' type. Coupling
is instead achieved by running the new 'createNonConformalCouples'
utility, which creates additional coupled patches of type
'nonConformalCyclic'. These appear in the 'constant/polyMesh/boundary'
file with zero faces; they are populated with faces in the finite volume
mesh during the connection process in NCC.
For a single couple, such as that which separates the rotating and
stationary sections of a mesh, the utility can be called using the
non-coupled patch names as arguments, e.g.
createNonConformalCouples -overwrite rotatingZoneInner rotatingZoneOuter
where 'rotatingZoneInner' and 'rotatingZoneOuter' are the names of the
patches.
For multiple couples, and/or couples with transformations,
'createNonConformalCouples' should be run without arguments. Settings
will then be read from a configuration file named
'system/createNonConformalCouplesDict'. See
'$FOAM_ETC/caseDicts/annotated/createNonConformalCouplesDict' for
examples.
Boundary conditions must be specified for the non-coupled patches. For a
couple where the patches fully overlap, boundary conditions
corresponding to a slip wall are typically applied to fields, i.e
'movingWallSlipVelocity' (or 'slip' if the mesh is stationary) for
velocity U, 'zeroGradient' or 'fixedFluxPressure' for pressure p, and
'zeroGradient' for other fields. For a couple with
partially-overlapping patches, boundary conditions are applied which
physically represent the non-overlapped region, e.g. a no-slip wall.
Boundary conditions also need to be specified for the
'nonConformalCyclic' patches created by 'createNonConformalCouples'. It
is generally recommended that this is done by including the
'$FOAM_ETC/caseDicts/setConstraintTypes' file in the 'boundaryField'
section of each of the field files, e.g.
boundaryField
{
#includeEtc "caseDicts/setConstraintTypes"
inlet
{
...
}
...
}
For moving mesh cases, it may be necessary to correct the mesh fluxes
that are changed as a result of the connection procedure. If the
connected patches do not conform perfectly to the mesh motion, then
failure to correct the fluxes can result in noise in the pressure
solution.
Correction for the mesh fluxes is enabled by the 'correctMeshPhi' switch
in the 'PIMPLE' (or equivalent) section of 'system/fvSolution'. When it
is enabled, solver settings are required for 'MeshPhi'. The solution
just needs to distribute the error enough to dissipate the noise. A
smooth solver with a loose tolerance is typically sufficient, e.g. the
settings in 'system/fvSolution' shown below:
solvers
{
MeshPhi
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-2;
relTol 0;
}
...
}
PIMPLE
{
correctMeshPhi yes;
...
}
The solution of 'MeshPhi' is an inexpensive computation since it is
applied only to a small subset of the mesh adjacent to the
couple. Conservation is maintained whether or not the mesh flux
correction is enabled, and regardless of the solution tolerance for
'MeshPhi'.
Advantages of NCC:
+ NCC maintains conservation which is required for many numerical
schemes and algorithms to operate effectively, in particular those
designed to maintain boundedness of a solution.
+ Closed-volume systems no longer suffer from accumulation or loss of
mass, poor convergence of the pressure equation, and/or concentration
of error in the reference cell.
+ Partially overlapped simulations are now possible on surfaces that are
not perfectly flat. The projection fills space so no overlaps or
spaces are generated inside contiguously overlapping sections, even if
those sections have sharp angles.
+ The finite volume faces created by NCC have geometrically accurate
centres. This makes the method second order accurate in space.
+ The polyhedral mesh no longer requires duplicate boundary faces to be
generated in order to run a partially overlapped simulation.
+ Lagrangian elements can now transfer across non-conformal couplings in
parallel.
+ Once the intersection has been computed and applied to the finite
volume mesh, it can use standard cyclic or processor cyclic finite
volume boundary conditions, with no need for additional patch types or
matrix interfaces.
+ Parallel communication is done using the standard
processor-patch-field system. This is more efficient than alternative
systems since it has been carefully optimised for use within the
linear solvers.
+ Coupled patches are disconnected prior to mesh motion and topology
change and reconnected afterwards. This simplifies the boundary
condition specification for mesh motion fields.
Resolved Bug Reports:
+ https://bugs.openfoam.org/view.php?id=663
+ https://bugs.openfoam.org/view.php?id=883
+ https://bugs.openfoam.org/view.php?id=887
+ https://bugs.openfoam.org/view.php?id=1337
+ https://bugs.openfoam.org/view.php?id=1388
+ https://bugs.openfoam.org/view.php?id=1422
+ https://bugs.openfoam.org/view.php?id=1829
+ https://bugs.openfoam.org/view.php?id=1841
+ https://bugs.openfoam.org/view.php?id=2274
+ https://bugs.openfoam.org/view.php?id=2561
+ https://bugs.openfoam.org/view.php?id=3817
Deprecation:
NCC replaces the functionality provided by AMI, ACMI and Repeat AMI.
ACMI and Repeat AMI are insufficiently reliable to warrant further
maintenance so are removed in an accompanying commit to OpenFOAM-dev.
AMI is more widely used so will be retained alongside NCC for the next
version release of OpenFOAM and then subsequently removed from
OpenFOAM-dev.
