Corrected a few issues with the utilisation of the tracking within the
nearWallFields function object. The tracking is now done over a
displacement from the initial location, which prevents trying to track
to a location outside the mesh when the patch face is warped and the
centre lies outside the tracking decomposition. Also fixed the end
criteria so that it does not suffer from round off error in the step
fraction.
The upshot of these changes is that the faces on which the near wall
cells were not being set are now being set properly, and uninitialised
data is no longer being written out.
Removed all the special handling for awkward particles from the
nearWallFields function object. The version 5+ tracking already handles
this more robustly.
Resolves bug-report https://bugs.openfoam.org/view.php?id=2728
A lot of methods were taking argument data which could be referenced or
generated from the parcel class at little or no additional cost. This
was confusing and generated the possibility of inconsistent data states.
Tracking data classes are no longer templated on the derived cloud type.
The advantage of this is that they can now be passed to sub models. This
should allow continuous phase data to be removed from the parcel
classes. The disadvantage is that every function which once took a
templated TrackData argument now needs an additional TrackCloudType
argument in order to perform the necessary down-casting.
Particle collisions with ACMI patches are now handled. The hit detects
whether the location is within the overlap or the coupled region and
recurses, calling the hit routine appropriate for the region.
The low level tracking methods are now more consistently named. There is
now a distinction between tracking to a face and hitting it. Function
object side effects have been moved out of the base layer and into the
parcels on which they are meaningful.
When an OpenFOAM simulation runs in parallel, the data for decomposed fields and
mesh(es) has historically been stored in multiple files within separate
directories for each processor. Processor directories are named 'processorN',
where N is the processor number.
This commit introduces an alternative "collated" file format where the data for
each decomposed field (and mesh) is collated into a single file, which is
written and read on the master processor. The files are stored in a single
directory named 'processors'.
The new format produces significantly fewer files - one per field, instead of N
per field. For large parallel cases, this avoids the restriction on the number
of open files imposed by the operating system limits.
The file writing can be threaded allowing the simulation to continue running
while the data is being written to file. NFS (Network File System) is not
needed when using the the collated format and additionally, there is an option
to run without NFS with the original uncollated approach, known as
"masterUncollated".
The controls for the file handling are in the OptimisationSwitches of
etc/controlDict:
OptimisationSwitches
{
...
//- Parallel IO file handler
// uncollated (default), collated or masterUncollated
fileHandler uncollated;
//- collated: thread buffer size for queued file writes.
// If set to 0 or not sufficient for the file size threading is not used.
// Default: 2e9
maxThreadFileBufferSize 2e9;
//- masterUncollated: non-blocking buffer size.
// If the file exceeds this buffer size scheduled transfer is used.
// Default: 2e9
maxMasterFileBufferSize 2e9;
}
When using the collated file handling, memory is allocated for the data in the
thread. maxThreadFileBufferSize sets the maximum size of memory in bytes that
is allocated. If the data exceeds this size, the write does not use threading.
When using the masterUncollated file handling, non-blocking MPI communication
requires a sufficiently large memory buffer on the master node.
maxMasterFileBufferSize sets the maximum size in bytes of the buffer. If the
data exceeds this size, the system uses scheduled communication.
The installation defaults for the fileHandler choice, maxThreadFileBufferSize
and maxMasterFileBufferSize (set in etc/controlDict) can be over-ridden within
the case controlDict file, like other parameters. Additionally the fileHandler
can be set by:
- the "-fileHandler" command line argument;
- a FOAM_FILEHANDLER environment variable.
A foamFormatConvert utility allows users to convert files between the collated
and uncollated formats, e.g.
mpirun -np 2 foamFormatConvert -parallel -fileHandler uncollated
An example case demonstrating the file handling methods is provided in:
$FOAM_TUTORIALS/IO/fileHandling
The work was undertaken by Mattijs Janssens, in collaboration with Henry Weller.
"pos" now returns 1 if the argument is greater than 0, otherwise it returns 0.
This is consistent with the common mathematical definition of the "pos" function:
https://en.wikipedia.org/wiki/Sign_(mathematics)
However the previous implementation in which 1 was also returned for a 0
argument is useful in many situations so the "pos0" has been added which returns
1 if the argument is greater or equal to 0. Additionally the "neg0" has been
added which returns 1 if if the argument is less than or equal to 0.
This function object reports the height of the interface above a set of
locations. It writes the height above the location, above the boundary,
and the point on the interface. It uses an integral approach, so if
there are multiple interfaces above or below a location, this method
will compute an average.
It can be enabled with the following entry in the system/controlDict:
functions
{
interfaceHeight1
{
type interfaceHeight;
libs ("libfieldFunctionObjects.so");
alpha alpha.water;
locations ((0 0 0) (10 0 0) (20 0 0));
}
}
This work was supported by Jan Kaufmann and Jan Oberhagemann at DNV GL.
terms of the local barycentric coordinates of the current tetrahedron,
rather than the global coordinate system.
Barycentric tracking works on any mesh, irrespective of mesh quality.
Particles do not get "lost", and tracking does not require ad-hoc
"corrections" or "rescues" to function robustly, because the calculation
of particle-face intersections is unambiguous and reproducible, even at
small angles of incidence.
Each particle position is defined by topology (i.e. the decomposed tet
cell it is in) and geometry (i.e. where it is in the cell). No search
operations are needed on restart or reconstruct, unlike when particle
positions are stored in the global coordinate system.
The particle positions file now contains particles' local coordinates
and topology, rather than the global coordinates and cell. This change
to the output format is not backwards compatible. Existing cases with
Lagrangian data will not restart, but they will still run from time
zero without any modification. This change was necessary in order to
guarantee that the loaded particle is valid, and therefore
fundamentally prevent "loss" and "search-failure" type bugs (e.g.,
2517, 2442, 2286, 1836, 1461, 1341, 1097).
The tracking functions have also been converted to function in terms
of displacement, rather than end position. This helps remove floating
point error issues, particularly towards the end of a tracking step.
Wall bounded streamlines have been removed. The implementation proved
incompatible with the new tracking algorithm. ParaView has a surface
LIC plugin which provides equivalent, or better, functionality.
Additionally, bug report <https://bugs.openfoam.org/view.php?id=2517>
is resolved by this change.
except turbulence and lagrangian which will also be updated shortly.
For example in the nonNewtonianIcoFoam offsetCylinder tutorial the viscosity
model coefficients may be specified in the corresponding "<type>Coeffs"
sub-dictionary:
transportModel CrossPowerLaw;
CrossPowerLawCoeffs
{
nu0 [0 2 -1 0 0 0 0] 0.01;
nuInf [0 2 -1 0 0 0 0] 10;
m [0 0 1 0 0 0 0] 0.4;
n [0 0 0 0 0 0 0] 3;
}
BirdCarreauCoeffs
{
nu0 [0 2 -1 0 0 0 0] 1e-06;
nuInf [0 2 -1 0 0 0 0] 1e-06;
k [0 0 1 0 0 0 0] 0;
n [0 0 0 0 0 0 0] 1;
}
which allows a quick change between models, or using the simpler
transportModel CrossPowerLaw;
nu0 [0 2 -1 0 0 0 0] 0.01;
nuInf [0 2 -1 0 0 0 0] 10;
m [0 0 1 0 0 0 0] 0.4;
n [0 0 0 0 0 0 0] 3;
if quick switching between models is not required.
To support this more convenient parameter specification the inconsistent
specification of seedSampleSet in the streamLine and wallBoundedStreamLine
functionObjects had to be corrected from
// Seeding method.
seedSampleSet uniform; //cloud; //triSurfaceMeshPointSet;
uniformCoeffs
{
type uniform;
axis x; //distance;
// Note: tracks slightly offset so as not to be on a face
start (-1.001 -0.05 0.0011);
end (-1.001 -0.05 1.0011);
nPoints 20;
}
to the simpler
// Seeding method.
seedSampleSet
{
type uniform;
axis x; //distance;
// Note: tracks slightly offset so as not to be on a face
start (-1.001 -0.05 0.0011);
end (-1.001 -0.05 1.0011);
nPoints 20;
}
which also support the "<type>Coeffs" form
// Seeding method.
seedSampleSet
{
type uniform;
uniformCoeffs
{
axis x; //distance;
// Note: tracks slightly offset so as not to be on a face
start (-1.001 -0.05 0.0011);
end (-1.001 -0.05 1.0011);
nPoints 20;
}
}
The standard naming convention for heat flux is "q" and this is used for the
conductive and convective heat fluxes is OpenFOAM. The use of "Qr" for
radiative heat flux is an anomaly which causes confusion, particularly for
boundary conditions in which "Q" is used to denote power in Watts. The name of
the radiative heat flux has now been corrected to "qr" and all models, boundary
conditions and tutorials updated.
e.g.
fieldMinMax fieldMinMax write:
min(T) = 291 in cell 255535 at location (-0.262546 -0.538933 1.00574) on processor 9
max(T) = 336.298 in cell 419031 at location (1.7468 0.758405 8.10989) on processor 1
min(mag(U)) = 0 in cell 14990 at location (-0.0824383 1.68479 1.5349) on processor 0
max(mag(U)) = 652.341 in cell 218284 at location (0.609849 0.167247 1.00091) on processor 12
defined by functionObjects, e.g. wallHeatFlux, wallShearStress and yPlus.
Patch contributed by Bruno Santos
Resolves bug-report http://bugs.openfoam.org/view.php?id=2353
postProcess -func MachNo
previously generated the warning
Executing functionObjects
--> FOAM Warning : functionObjects::MachNo MachNo cannot find required field U
which is incorrect; the field 'U' is available but the
thermophysicalProperties is not. Now 'postProcess' generates the
warning:
Executing functionObjects
--> FOAM Warning : functionObjects::MachNo MachNo cannot find required object thermophysicalProperties of type fluidThermo
--> FOAM Warning : functionObjects::MachNo MachNo failed to execute.
Resolves bug-report http://bugs.openfoam.org/view.php?id=2352
The operation can be applied to any volume or surface fields generating a
volume or surface scalar field.
Example of function object specification:
\verbatim
Ttot
{
type add;
libs ("libfieldFunctionObjects.so");
fields (T Tdelta);
result Ttot;
executeControl writeTime;
writeControl writeTime;
}
\endverbatim
Also refactored functionObjects::fieldsExpression to avoid code
duplication between the 'add' and 'subtract' functionObjects.
The operation can be applied to any volume or surface fields generating a
volume or surface scalar field.
Example of function object specification:
\verbatim
Tdiff
{
type subtract;
libs ("libfieldFunctionObjects.so");
fields (T Tmean);
result Tdiff;
executeControl writeTime;
writeControl writeTime;
}
\endverbatim
