Lagrangian injections now have a 'uniformParcelSize' control, which
specifies what size of the parcels is kept uniform during a given time
step. This control can be set to 'nParticles', 'surfaceArea' or
'volume'. The particle sizes, by contrast, are specified by the size
distribution.
For example, if 'uniformParcelSize nParticles;' is specified then all
parcels introduced at a given time will have the same number of
particles. Every particle in a parcel has the same properties, including
diameter. So, in this configuration, the larger diameter parcels contain
a much larger fraction of the total particulate volume than the smaller
diameter ones. This may be undesirable as the effect of a parcel on the
simulation might be more in proportion with its volume than with the
number of particles it represents. It might be preferable to create a
greater proportion of large diameter parcels so that their more
significant effect is represented by a finer Lagrangian discretisation.
This can be achieved by setting 'uniformParcelSize volume;'. A setting
of 'uniformParcelSize surfaceArea;' might be appropriate if the limiting
effect of a Lagrangian element scales with its surface area; interfacial
evaporation, for example.
Previously, this control was provided by 'parcelBasisType'. However,
this control also effectively specified the size exponent of the
supplied distribution. This interdependence was not documented and was
problematic in that it coupled physical and numerical controls.
'parcelBasisType' has been removed, and the size exponent of the
distribution is now specified independently of the new
'uniformParcelSize' control along with the rest of the distribution
coefficients or data. See the previous commit for details.
It is still possible to specify a fixed number of particles per parcel
using the 'nParticle' control. The presence of this control is used to
determine whether or not the number of particles per parcel is fixed, so
a 'fixed' basis type is no longer needed.
A number of bugs have been fixed with regards to lack of
interoperability between the various settings in the injection models.
'uniformParcelSize' can be changed freely and the number of parcels and
amount of mass that an injector introduces will not change (this was not
true of 'parcelBasisType'). Redundant settings are no longer read by the
injection models; e.g., mass is not read if the number of particles per
parcel is fixed, duration is not specified for steady tracking, etc...
The 'inflationInjection' model has been removed as there are no examples
of its usage, its purpose was not clearly documented, and it was not
obvious how it should be updated as a result of these changes.
This new class hierarchy replaces the distributions previously provided
by the Lagrangian library.
All distributions (except fixedValue) now require a "size exponent", Q,
to be specified along with their other coefficients. If a distribution's
CDF(x) (cumulative distribution function) represents what proportion of
the distribution takes a value below x, then Q determines what is meant
by "proportion":
- If Q=0, then "proportion" means the number of sampled values expected
to be below x divided by the total number of sampled values.
- If Q=3, then "proportion" means the expected sum of sampled values
cubed for values below x divided by the total sum of values cubed. If
x is a length, then this can be interpreted as a proportion of the
total volume of sampled objects.
- If Q=2, and x is a length, then the distribution might represent the
proportion of surface area, and so on...
In addition to the user-specification of Q defining what size the given
distribution relates to, an implementation that uses a distribution can
also programmatically define a samplingQ to determine what sort of
sample is being constructed; whether the samples should have an equal
number (sampleQ=0), volume (sampleQ=3), area (sampleQ=2), etc...
A number of fixes to the distributions have been made, including fixing
some fundamental bugs in the returned distribution of samples, incorrect
calculation of the distribution means, renaming misleadingly named
parameters, and correcting some inconsistencies in the way in which
tabulated PDF and CDF data was processed. Distributions no longer
require their parameters to be defined in a sub-dictionary, but a
sub-dictionary is still supported for backwards compatibility.
The distributions can now generate their PDF-s as well as samples, and a
test application has been added (replacing two previous applications),
which thoroughly checks consistency between the PDF and the samples for
a variety of combinations of values of Q and sampleQ.
Backwards incompatible changes are as follows:
- The standard deviation keyword for the normal (and multi-normal)
distribution is now called 'sigma'. Previously this was 'variance',
which was misleading, as the value is a standard deviation.
- The 'massRosinRammler' distribution has been removed. This
functionality is now provided by the standard 'RosinRammler'
distributon with a Q equal to 0, and a sampleQ of 3.
- The 'general' distribution has been split into separate distributions
based on whether PDF or CDF data is provided. These distributions are
called 'tabulatedDensity' and 'tabulatedCumulative', respectively.
This function outputs a graph of a cloud's particle and parcel size
distributions. It can be enabled by putting the following settings in
the 'cloudFunctions' section of the cloud's properties file:
sizeDistribution1
{
type sizeDistribution;
nPoints 40;
setFormat raw;
}
The calculation of the diffusion number has been put into a form
consistent with finite-volume, rather than the finite-difference form
that was used previously.
This difference in formulations is analogus to that of the Courant
number in the fluid solvers. Whilst a textbook will typically define the
courant number as equal to 'U*deltaT/deltaX', in a finite-volume context
it is more appropriate to define it as 'Sum(phi)/V*deltaT' (where 'Sum'
is a sum over the cell's faces). Similarly, the finite-difference
Fourier number, 'kappa/rho/Cp*deltaT/deltaX^2', is more consistently
expressed for finite-volume as 'Sum(Sf*kappa*deltaX)/(V*rho*Cp)*deltaT'.
This makes the calculation of the diffusion number less sensitive to the
presence of small, poor quality faces, and therefore makes time-step
adjustment more robust on arbitrary polyhedral meshes.
This change relaxes the previous restriction that mappedWall patches
cannot have transformation. It permits cyclic multi-region simulations
in which the cyclic plane lies on the interface between regions.
The mappedWall still differs from the mapped patch in that it is assumed
to be untransformed unless a transformation is explicitly specified. The
mapped patch, by contrast, will attempt to automatically calculate a
transformation from the geometry of the patches in the same way as is
done for cyclics.
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'
Now the -allLibs option loads all the libraries without listing them to reduce
the amount of output when it is not needed and the new -listAllLibs option loads
all the libraries and lists them as they are loaded which may be useful to find
libraries which do not load due to duplicate entries for example.
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;
}
The parcel transfer occurs from the cloudFilmTransfer surfaceFilmModel specified
in the <fluid> region constant/<fluid>/cloudProperties dictionary:
.
.
.
libs ("libfilmCloudTransfer.so");
.
.
.
surfaceFilmModel cloudFilmTransfer;
and the film filmCloudTransfer specified in the <film> region
constant/<film>/fvModels dictionary:
.
.
.
filmCloudTransfer
{
type filmCloudTransfer;
libs ("libfilmCloudTransfer.so");
}
For an example of cloud->film->VoF transfer see the
tutorials/modules/multiRegion/film/cylinder tutorial case.
Note that parcel transfer from film to Lagrangian cloud is not yet supported,
this will be added soon.
The two-phase VoF alphaContactAngleFvPatchScalarField class has been renamed
contactAngleFvPatchScalarField to avoid a name clash with the multiphaseEuler
version of alphaContactAngleFvPatchScalarField so that both VoF and
multiphaseEuler solver modules may be used in different regions of a
foamMultiRun simulation.
foamToC: New run-time selection table of contents printing and interrogation utility
The new solver modules cannot provide the equivalent functionality of the -list
options available in the solver applications so foamToC has been developed as a
better, more general and flexible alternative, providing a means to print any or
all run-time selection tables in any or all libraries and search the tables for
any particular entries and print which library files the corresponding tables
are in, e.g.
foamToC -solver fluid -table fvPatchScalarField
Contents of table fvPatchScalarField, base type fvPatchField:
advective libfiniteVolume.so
calculated libfiniteVolume.so
codedFixedValue libfiniteVolume.so
codedMixed libfiniteVolume.so
compressible::alphatJayatillekeWallFunctionlibthermophysicalTransportModels.so
compressible::alphatWallFunction libthermophysicalTransportModels.so
compressible::thermalBaffle1D<eConstSolidThermoPhysics>libthermophysicalTransportModels.so
compressible::thermalBaffle1D<ePowerSolidThermoPhysics>libthermophysicalTransportModels.so
compressible::turbulentTemperatureCoupledBaffleMixedlibthermophysicalTransportModels.so
compressible::turbulentTemperatureRadCoupledMixedlibthermophysicalTransportModels.so
.
.
.
foamToC -solver fluid -search compressible::alphatWallFunction
compressible::alphatWallFunction is in tables
fvPatchField
fvPatchScalarField libthermophysicalTransportModels.so
and the very useful -allLibs option allows ALL libraries to be searched to find
in which table and which library file a particular model in in for example:
foamToC -allLibs -search phaseTurbulenceStabilisation
Loading libraries:
libtwoPhaseSurfaceTension.so
libcv2DMesh.so
libODE.so
.
.
.
phaseTurbulenceStabilisation is in tables
fvModel libmultiphaseEulerFoamFvModels.so
Application
foamToC
Description
Run-time selection table of contents printing and interrogation.
The run-time selection tables are populated by the optionally specified
solver class and any additional libraries listed in the \c -libs option or
all libraries using the \c -allLibs option. Once populated the tables can
be searched and printed by a range of options listed below. Table entries
are printed with the corresponding library they are in to aid selection
and the addition of \c libs entries to ensure availability to the solver.
Usage
\b foamToC [OPTION]
- \par -solver \<name\>
Specify the solver class
- \par -libs '(\"lib1.so\" ... \"libN.so\")'
Specify the additional libraries to load
- \par -allLibs
Load all libraries
- \par switches,
List all available debug, info and optimisation switches
- \par all,
List the contents of all the run-time selection tables
- \par tables
List the run-time selection table names (this is the default action)
- \par table \<name\>
List the contents of the specified table or the list sub-tables
- \par search \<name\>
Search for and list the tables containing the given entry
- \par scalarBCs,
List scalar field boundary conditions (fvPatchField<scalar>)
- \par vectorBCs,
List vector field boundary conditions (fvPatchField<vector>)
- \par functionObjects,
List functionObjects
- \par fvModels,
List fvModels
- \par fvConstraints,
List fvConstraints
Example usage:
- Print the list of scalar boundary conditions (fvPatchField<scalar>)
provided by the \c fluid solver without additional libraries:
\verbatim
foamToC -solver fluid -scalarBCs
\endverbatim
- Print the list of RAS momentum transport models provided by the
\c fluid solver:
\verbatim
foamToC -solver fluid -table RAScompressibleMomentumTransportModel
\endverbatim
- Print the list of functionObjects provided by the
\c multicomponentFluid solver with the libfieldFunctionObjects.so
library:
\verbatim
foamToC -solver multicomponentFluid \
-libs '("libfieldFunctionObjects.so")' -functionObjects
\endverbatim
- Print a complete list of all run-time selection tables:
\verbatim
foamToC -allLibs -tables
or
foamToC -allLibs
\endverbatim
- Print a complete list of all entries in all run-time selection tables:
\verbatim
foamToC -allLibs -all
\endverbatim
executed with foamRun for single region simulations of foamMultiRun for
multi-region simulations. Replaces driftFluxFoam and all the corresponding
tutorials have been updated and moved to
tutorials/modules/incompressibleDriftFlux.
Class
Foam::solvers::incompressibleDriftFlux
Description
Solver module for 2 incompressible fluids using the mixture approach with
the drift-flux approximation for relative motion of the phases, with
optional mesh motion and mesh topology changes including adaptive
re-meshing.
The momentum and other fluid properties are of the "mixture" and a single
momentum equation is solved with mixture transport modelling in which a
single laminar, RAS or LES model is selected to model the momentum stress.
Uses the flexible PIMPLE (PISO-SIMPLE) solution for time-resolved and
pseudo-transient and steady simulations.
Optional fvModels and fvConstraints are provided to enhance the simulation
in many ways including adding various sources, Lagrangian
particles, surface film etc. and constraining or limiting the solution.
SourceFiles
incompressibleDriftFlux.C
See also
Foam::solvers::VoFSolver
Foam::solvers::twoPhaseVoFSolver
Foam::solvers::compressibleVoF
