Description
Evolves a passive scalar transport equation.
- To specify the field name set the \c field entry
- To employ the same numerical schemes as another field set
the \c schemesField entry,
- The \c diffusivity entry can be set to \c none, \c constant, \c viscosity
- A constant diffusivity is specified with the \c D entry,
- If a momentum transport model is available and the \c viscosity
diffusivety option specified an effective diffusivity may be constructed
from the laminar and turbulent viscosities using the diffusivity
coefficients \c alphal and \c alphat:
\verbatim
D = alphal*nu + alphat*nut
\endverbatim
Example:
\verbatim
#includeFunc scalarTransport(T, alphaD=1, alphaDt=1)
\endverbatim
For incompressible flow the passive scalar may optionally be solved with the
MULES limiter and sub-cycling or semi-implicit in order to maintain
boundedness, particularly if a compressive, PLIC or MPLIC convection
scheme is used.
Example:
\verbatim
#includeFunc scalarTransport(tracer, diffusion=none)
with scheme specification:
div(phi,tracer) Gauss interfaceCompression vanLeer 1;
and solver specification:
tracer
{
nCorr 1;
nSubCycles 3;
MULESCorr no;
nLimiterIter 5;
applyPrevCorr yes;
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-8;
relTol 0;
diffusion
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-8;
relTol 0;
}
}
\endverbatim
Packaged function objects can now be deployed equally effectively by
(a) using a locally edited copy of the configuration file, or by
(b) passing parameters as arguments to the global configuration file.
For example, to post-process the pressure field "p" at a single location
"(1 2 3)", the user could first copy the "probes" packaged function
object file to their system directory by calling "foamGet probes". They
could then edit the file to contain the following entries:
points ((1 2 3));
field p;
The function object can then be executed by the postProcess application:
postProcess -func probes
Or it can be called at run-time, by including from within the functions
section of the system/controlDict file:
#includeFunc probes
Alternatively, the field and points parameters could be passed as
arguments either to the postProcess application by calling:
postProcess -func "probes(points=((1 2 3)), p)"
Or by using the #includeFunc directive:
#includeFunc probes(points=((1 2 3)), p)
In both cases, mandatory parameters that must be either edited or
provided as arguments are denoted in the configuration files with
angle-brackets, e.g.:
points (<points>);
Many of the packaged function objects have been split up to make them
more specific to a particular use-case. For example, the "surfaces"
function has been split up into separate functions for each surface
type; "cutPlaneSurface", "isoSurface", and "patchSurface". This
splitting means that the packaged functions now only contain one set of
relevant parameters so, unlike previously, they now work effectively
with their parameters passed as arguments. To ensure correct usage, all
case-dependent parameters are considered mandatory.
For example, the "streamlines" packaged function object has been split
into specific versions; "streamlinesSphere", "streamlinesLine",
"streamlinesPatch" and "streamlinesPoints". The name ending denotes the
seeding method. So, the following command creates ten streamlines with
starting points randomly seeded within a sphere with a specified centre
and radius:
postProcess -func "streamlinesSphere(nPoints=10, centre=(0 0 0), radius=1)"
The equivalent #includeFunc approach would be:
#includeFunc streamlinesSphere(nPoints=10, centre=(0 0 0), radius=1)
When passing parameters as arguments, error messages report accurately
which mandatory parameters are missing and provide instructions to
correct the format of the input. For example, if "postProcess -func
graphUniform" is called, then the code prints the following error message:
--> FOAM FATAL IO ERROR:
Essential value for keyword 'start' not set
Essential value for keyword 'end' not set
Essential value for keyword 'nPoints' not set
Essential value for keyword 'fields' not set
In function entry:
graphUniform
In command:
postProcess -func graphUniform
The function entry should be:
graphUniform(start = <point>, end = <point>, nPoints = <number>, fields = (<fieldNames>))
file: controlDict/functions/graphUniform from line 15 to line 25.
As always, a full list of all packaged function objects can be obtained
by running "postProcess -list", and a description of each function can
be obtained by calling "foamInfo <functionName>". An example case has
been added at "test/postProcessing/channel" which executes almost all
packaged function objects using both postProcess and #includeFunc. This
serves both as an example of syntax and as a unit test for maintenance.
The standard set of Lagrangian clouds are now selectable at run-time.
This means that a solver that supports Lagrangian modelling can now use
any type of cloud (with some restrictions). Previously, solvers were
hard-coded to use specific cloud modelling. In addition, a cloud-list
structure has been added so that solvers may select multiple clouds,
rather than just one.
The new system is controlled as follows:
- If only a single cloud is required, then the settings for the
Lagrangian modelling should be placed in a constant/cloudProperties
file.
- If multiple clouds are required, then a constant/clouds file should be
created containing a list of cloud names defined by the user. Each
named cloud then reads settings from a corresponding
constant/<cloudName>Properties file. Clouds are evolved sequentially
in the order in which they are listed in the constant/clouds file.
- If no clouds are required, then the constant/cloudProperties file and
constant/clouds file should be omitted.
The constant/cloudProperties or constant/<cloudName>Properties files are
the same as previous cloud properties files; e.g.,
constant/kinematicCloudProperties or constant/reactingCloud1Properties,
except that they now also require an additional top-level "type" entry
to select which type of cloud is to be used. The available options for
this entry are:
type cloud; // A basic cloud of solid
// particles. Includes forces,
// patch interaction, injection,
// dispersion and stochastic
// collisions. Same as the cloud
// previously used by
// rhoParticleFoam
// (uncoupledKinematicParticleFoam)
type collidingCloud; // As "cloud" but with resolved
// collision modelling. Same as the
// cloud previously used by DPMFoam
// and particleFoam
// (icoUncoupledKinematicParticleFoam)
type MPPICCloud; // As "cloud" but with MPPIC
// collision modelling. Same as the
// cloud previously used by
// MPPICFoam.
type thermoCloud; // As "cloud" but with
// thermodynamic modelling and heat
// transfer with the carrier phase.
// Same as the limestone cloud
// previously used by
// coalChemistryFoam.
type reactingCloud; // As "thermoCloud" but with phase
// change and mass transfer
// coupling with the carrier
// phase. Same as the cloud
// previously used in fireFoam.
type reactingMultiphaseCloud; // As "reactingCloud" but with
// particles that contain multiple
// phases. Same as the clouds
// previously used in
// reactingParcelFoam and
// simpleReactingParcelFoam and the
// coal cloud used in
// coalChemistryFoam.
type sprayCloud; // As "reactingCloud" but with
// additional spray-specific
// collision and breakup modelling.
// Same as the cloud previously
// used in sprayFoam and
// engineFoam.
The first three clouds are not thermally coupled, so are available in
all Lagrangian solvers. The last four are thermally coupled and require
access to the carrier thermodynamic model, so are only available in
compressible Lagrangian solvers.
This change has reduced the number of solvers necessary to provide the
same functionality; solvers that previously differed only in their
Lagrangian modelling can now be combined. The Lagrangian solvers have
therefore been consolidated with consistent naming as follows.
denseParticleFoam: Replaces DPMFoam and MPPICFoam
reactingParticleFoam: Replaces sprayFoam and coalChemistryFoam
simpleReactingParticleFoam: Replaces simpleReactingParcelFoam
buoyantReactingParticleFoam: Replaces reactingParcelFoam
fireFoam and engineFoam remain, although fireFoam is likely to be merged
into buoyantReactingParticleFoam in the future once the additional
functionality it provides is generalised.
Some additional minor functionality has also been added to certain
solvers:
- denseParticleFoam has a "cloudForceSplit" control which can be set in
system/fvOptions.PIMPLE. This provides three methods for handling the
cloud momentum coupling, each of which have different trade-off-s
regarding numerical artefacts in the velocity field. See
denseParticleFoam.C for more information, and also bug report #3385.
- reactingParticleFoam and buoyantReactingParticleFoam now support
moving mesh in order to permit sharing parts of their implementation
with engineFoam.
providing the shear-stress term in the momentum equation for incompressible and
compressible Newtonian, non-Newtonian and visco-elastic laminar flow as well as
Reynolds averaged and large-eddy simulation of turbulent flow.
The general deviatoric shear-stress term provided by the MomentumTransportModels
library is named divDevTau for compressible flow and divDevSigma (sigma =
tau/rho) for incompressible flow, the spherical part of the shear-stress is
assumed to be either included in the pressure or handled separately. The
corresponding stress function sigma is also provided which in the case of
Reynolds stress closure returns the effective Reynolds stress (including the
laminar contribution) or for other Reynolds averaged or large-eddy turbulence
closures returns the modelled Reynolds stress or sub-grid stress respectively.
For visco-elastic flow the sigma function returns the effective total stress
including the visco-elastic and Newtonian contributions.
For thermal flow the heat-flux generated by thermal diffusion is now handled by
the separate ThermophysicalTransportModels library allowing independent run-time
selection of the heat-flux model.
During the development of the MomentumTransportModels library significant effort
has been put into rationalising the components and supporting libraries,
removing redundant code, updating names to provide a more logical, consistent
and extensible interface and aid further development and maintenance. All
solvers and tutorials have been updated correspondingly and backward
compatibility of the input dictionaries provided.
Henry G. Weller
CFD Direct Ltd.
This is like the scalarTrasport function except that the transported
scalar is confined to a single phase of a multiphase simulation. In
addition to the usual specification for the scalarTransport function
(i.e., a field, schemes and solution parameters), the user needs to
specify the phase-flux or a pressure field which can be used to generate
it.
Example usage for interFoam:
phaseScalarTransport1
{
type phaseScalarTransport;
libs ("libsolverFunctionObjects.so");
field s.water;
p p_rgh;
}
Example usage for reactingTwoPhaseEulerFoam:
phaseScalarTransport1
{
type phaseScalarTransport;
libs ("libsolverFunctionObjects.so");
field s.water;
alphaPhi alphaRhoPhi.water;
rho thermo:rho.water;
}
The function will write out both the per-unit-phase field that is solved
for (s.water in the above examples) and also the mixture-total field
(alphaS.water), which is often more convenient for post-processing.
