The new fvModels is a general interface to optional physical models in the
finite volume framework, providing sources to the governing conservation
equations, thus ensuring consistency and conservation. This structure is used
not only for simple sources and forces but also provides a general run-time
selection interface for more complex models such as radiation and film, in the
future this will be extended to Lagrangian, reaction, combustion etc. For such
complex models the 'correct()' function is provided to update the state of these
models at the beginning of the PIMPLE loop.
fvModels are specified in the optional constant/fvModels dictionary and
backward-compatibility with fvOption is provided by reading the
constant/fvOptions or system/fvOptions dictionary if present.
The new fvConstraints is a general interface to optional numerical constraints
applied to the matrices of the governing equations after construction and/or to
the resulting field after solution. This system allows arbitrary changes to
either the matrix or solution to ensure numerical or other constraints and hence
violates consistency with the governing equations and conservation but it often
useful to ensure numerical stability, particularly during the initial start-up
period of a run. Complex manipulations can be achieved with fvConstraints, for
example 'meanVelocityForce' used to maintain a specified mean velocity in a
cyclic channel by manipulating the momentum matrix and the velocity solution.
fvConstraints are specified in the optional system/fvConstraints dictionary and
backward-compatibility with fvOption is provided by reading the
constant/fvOptions or system/fvOptions dictionary if present.
The separation of fvOptions into fvModels and fvConstraints provides a rational
and consistent separation between physical and numerical models which is easier
to understand and reason about, avoids the confusing issue of location of the
controlling dictionary file, improves maintainability and easier to extend to
handle current and future requirements for optional complex physical models and
numerical constraints.
Specifying a plane with which to subset feature edges is now done using
the same dictionary syntax used elsewhere in OpenFOAM. For example, in
system/surfaceFeaturesDict:
subsetFeatures
{
// Include only edges that intersect the plane
plane
{
planeType pointAndNormal;
point (0 0 0);
normal (1 0 0);
}
...
}
A number of fvOptions that apply to a user-derined field can now
automatically work what primitive type they apply to. These options can
apply to any field type, and in some cases even multiple fields of
differing type. Example usage of the options to which this change
applies are shown below:
codedSource1
{
type codedSource;
name codedSource1;
field h;
...
}
fixedValueConstraint1
{
type fixedValueConstraint;
fieldValues
{
R (1 0 0 1 0 1);
epsilon 150;
}
...
}
phaseLimitStabilization11
{
type phaseLimitStabilization;
field sigma.liquid;
...
}
Previously to apply to a given type, these options had to be selected
with the name of the type prepended to the option name (e.g., "type
symmTensorPhaseLimitStabilization;") and those that operated on multiple
fields were restricted to those fields being of the same type.
A number of other options have had improvements made to their handling
of user specification of fields. Where possible, the option will now
attempt to work out what field the option applies to automatically. The
following options, therefore, no longer require "field" or "fields"
entries:
actuationDiskSource
buoyancyEnergy
buoyancyForce
meanVelocityForce
rotorDiskSource
volumeFractionSource
constantHeatTransfer
function2HeatTransfer
variableHeatTransfer
Non-standard field names can be overridden in the same way as in
boundary conditions; e.g., the velocity name can be overridden with a "U
<UName>;" entry if it does not have the default name, "U". The name of
the energy field is now always determined from the thermodynamics
model and should always be correct. Some options that can be applied to
an individual phase also support a "phase <phaseName>;" entry;
fvOptions field-name handling has been rewritten to increase its
flexibility and to improve warning messages. The flexibility now allows
for options that apply to all fields, or all fields of a given phase,
rather than being limited to a specific list of field names. Messages
warning about options that have not been applied now always print just
once per time-step.
Originally the only supported geometry specification were triangulated surfaces,
hence the name of the directory: constant/triSurface, however now that other
surface specifications are supported and provided it is much more logical that
the directory is named accordingly: constant/geometry. All tutorial and
template cases have been updated.
Note that backward compatibility is provided such that if the constant/geometry
directory does not exist but constant/triSurface does then the geometry files
are read from there.
The phase-change functionality in interPhaseChangeFoam has been generalised and
moved into the run-time selectable twoPhaseChange library included into
interFoam providing optional phase-change. The three cavitation models provided
in interPhaseChangeFoam are now included in the twoPhaseChange library and the
two interPhaseChangeFoam cavitation tutorials updated for interFoam.
interPhaseChangeFoam has been replaced by a user redirection script which prints
the following message:
The interPhaseChangeFoam solver has solver has been replaced by the more general
interFoam solver, which now supports phase-change using the new twoPhaseChange
models library.
To run with with phase-change create a constant/phaseChangeProperties dictionary
containing the phase-change model specification, e.g.
phaseChangeModel SchnerrSauer;
pSat 2300; // Saturation pressure
See the following cases for an example converted from interPhaseChangeFoam:
$FOAM_TUTORIALS/multiphase/interFoam/laminar/cavitatingBullet
$FOAM_TUTORIALS/multiphase/interFoam/RAS/propeller
End points of topoSet cylinder sources should now be specified as
"point1" and "point2", which is consistent with other parts of the code.
The previous keywords, "p1" and "p2" have been retained for backwards
compatibility but may be removed in future.
A volumetric flow rate through a tri-surface can now be obtained using
the volumetricFlowRateTriSurface preconfigured function object, using
the following entry in system/controlDict:
fuctions
{
#includeFunc "volumetricFlowRateTriSurface(name=surface.stl)"
}
Where "surface.stl" is a tri-surface file in the constant/triSurface
directory. An example of this has been added to the
incompressible/pimpleFoam/RAS/impeller tutorial case.
Note that when possible, it is preferable to use the flowRatePatch or
flowRateFaceZone functions, as these make direct use of the flux and
therefore report a value that is exactly that computed by the solver.
volumetricFlowRateTriSurface, by contrast, does interpolation of the
velocity field which introduces error.
In addition, a minor fix has been made to the underlying
surfaceFieldValue function object so that it does not need a zone/set
name when values on a searchable surface are requested.
It is better to not select and instantiate a model, fvOption etc. than to create
it and set it inactive as the creation process requires reading of settings,
parameters, fields etc. with all the associated specification and storage
without being used. Also the incomplete implementation added a lot of
complexity in the low-level operation of models introducing a significant
maintenance overhead and development overhead for new models.
There are now three possible code entries for the scalarCodedSource,
vectorCodedSource, etc..., fvOptions. These are `codeAddSup` for basic
sources, `codeAddRhoSup` for compressible sources, and
`codeAddAlphaRhoSup` for phase (compressible) sources.
Previously `codeAddSup` was used for both basic and compressible
sources, and phase sources were not implemented. This meant that whilst
a compressible source could be created, it could not make use of the
`rho` argument or the basic source function would fail to compile.
Solid thermo no longer requires a pressure field, so solid regions of
chtMultiRegionFoam cases no longer need a 0/<solidRegionName>/p file.
In order for solidThermo to continue to use heThermo and the low level
thermo classes, it now constructs a uniformGeometricScalarField for the
pressure with the value NaN. This is passed into the low-level thermo
models by heThermo. The enforces the requirement that low-level thermo
models used by solidThermo should have no pressure dependence. If an
instantiation is made with pressure dependence, the code will fail with
a floating point error.
Most fvOptions change the state of the fields and equations they are applied to
but do not change internal state so it makes more sense that the interface is
const, consistent with MeshObjects. For the few fvOptions which do maintain a
changing state the member data is now mutable.
There is now only one -listSwitches argument available to the
applications; -listUnsetSwitches and -listRegisteredSwitches have been
removed. -listSwitches prints everything, now also including the values.
It also categorises the output based on whether the switch has a
default, if it has the same value as that default, and whether or not it
is registered with a re-reader.
The list of debug switches in etc/controlDict has been reduced to only
the switches which have non-zero values. In general the list of valid
switches varies per application and per library, so it is not possible
to keep a single definitive list of all switches. The -listSwitches
argument provides the definitive list on a per applicaton basis.
Setting of defaults for named enum optimisation switches has been added.
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.
The new optional 'slash' scoping syntax is now the default and provides a more
intuitive and flexible syntax than the previous 'dot' syntax, corresponding to
the common directory/file access syntax used in UNIX, providing support for
reading entries from other dictionary files.
In the 'slash' syntax
'/' is the scope operator
'../' is the parent dictionary scope operator
'!' is the top-level dictionary scope operator
Examples:
internalField 3.4;
active
{
type fixedValue;
value.air $internalField;
}
inactive
{
type anotherFixedValue;
value $../active/value.air;
anotherValue $!active/value.air;
sub
{
value $../../active/value.air;
anotherValue $!active/value.air;
}
}
"U.*"
{
solver GAMG;
}
e.air
{
$U.air;
}
external
{
value $testSlashDict2!active/value.air;
}
active2
{
$testSlashDict2!active;
}
If there is a part of the keyword before the '!' then this is taken to be the
file name of the dictionary from which the entry will be looked-up using the
part of the keyword after the '!'. For example given a file testSlashDict containing
internalField 5.6;
active
{
type fixedValue;
value.air $internalField;
}
entries from it can be read directly from another file, e.g.
external
{
value $testSlashDict2!active/value.air;
}
active2
{
$testSlashDict2!active;
}
which expands to
external
{
value 5.6;
}
active2
{
type fixedValue;
value.air 5.6;
}
These examples are provided in applications/test/dictionary.
The the default syntax can be changed from 'slash' to 'dot' in etc/controlDict
to revert to the previous behaviour:
OptimisationSwitches
{
.
.
.
// Default dictionary scoping syntax
inputSyntax slash; // Change to dot for previous behaviour
}
or within a specific dictionary by adding the entry
See applications/test/dictionary/testDotDict.
The reactingtTwoPhaseEulerFoam solver has been replaced by the more general
multiphaseEulerFoam solver which supports two-phase and multiphase systems
containing fluid and stationary phases, compressible or incompressible, with
heat and mass transfer, reactions, size distribution and all the usual phase
interaction and transfer models.
All reactingtTwoPhaseEulerFoam tutorials have been ported to multiphaseEulerFoam
to demonstrate two-phase capability with a wide range of phase and
phase-interaction models.
When running with two-phases the optional referencePhase entry in
phaseProperties can be used to specify which phase fraction should not be
solved, providing compatibility with reactingtTwoPhaseEulerFoam, see
tutorials/multiphase/multiphaseEulerFoam/RAS/fluidisedBed
tutorials/multiphase/multiphaseEulerFoam/laminar/bubbleColumn
for examples.
