to provide a single consistent code and user interface to the specification of
physical properties in both single-phase and multi-phase solvers. This redesign
simplifies usage and reduces code duplication in run-time selectable solver
options such as 'functionObjects' and 'fvModels'.
* physicalProperties
Single abstract base-class for all fluid and solid physical property classes.
Physical properties for a single fluid or solid within a region are now read
from the 'constant/<region>/physicalProperties' dictionary.
Physical properties for a phase fluid or solid within a region are now read
from the 'constant/<region>/physicalProperties.<phase>' dictionary.
This replaces the previous inconsistent naming convention of
'transportProperties' for incompressible solvers and
'thermophysicalProperties' for compressible solvers.
Backward-compatibility is provided by the solvers reading
'thermophysicalProperties' or 'transportProperties' if the
'physicalProperties' dictionary does not exist.
* phaseProperties
All multi-phase solvers (VoF and Euler-Euler) now read the list of phases and
interfacial models and coefficients from the
'constant/<region>/phaseProperties' dictionary.
Backward-compatibility is provided by the solvers reading
'thermophysicalProperties' or 'transportProperties' if the 'phaseProperties'
dictionary does not exist. For incompressible VoF solvers the
'transportProperties' is automatically upgraded to 'phaseProperties' and the
two 'physicalProperties.<phase>' dictionary for the phase properties.
* viscosity
Abstract base-class (interface) for all fluids.
Having a single interface for the viscosity of all types of fluids facilitated
a substantial simplification of the 'momentumTransport' library, avoiding the
need for a layer of templating and providing total consistency between
incompressible/compressible and single-phase/multi-phase laminar, RAS and LES
momentum transport models. This allows the generalised Newtonian viscosity
models to be used in the same form within laminar as well as RAS and LES
momentum transport closures in any solver. Strain-rate dependent viscosity
modelling is particularly useful with low-Reynolds number turbulence closures
for non-Newtonian fluids where the effect of bulk shear near the walls on the
viscosity is a dominant effect. Within this framework it would also be
possible to implement generalised Newtonian models dependent on turbulent as
well as mean strain-rate if suitable model formulations are available.
* visosityModel
Run-time selectable Newtonian viscosity model for incompressible fluids
providing the 'viscosity' interface for 'momentumTransport' models.
Currently a 'constant' Newtonian viscosity model is provided but the structure
supports more complex functions of time, space and fields registered to the
region database.
Strain-rate dependent non-Newtonian viscosity models have been removed from
this level and handled in a more general way within the 'momentumTransport'
library, see section 'viscosity' above.
The 'constant' viscosity model is selected in the 'physicalProperties'
dictionary by
viscosityModel constant;
which is equivalent to the previous entry in the 'transportProperties'
dictionary
transportModel Newtonian;
but backward-compatibility is provided for both the keyword and model
type.
* thermophysicalModels
To avoid propagating the unnecessary constructors from 'dictionary' into the
new 'physicalProperties' abstract base-class this entire structure has been
removed from the 'thermophysicalModels' library. The only use for this
constructor was in 'thermalBaffle' which now reads the 'physicalProperties'
dictionary from the baffle region directory which is far simpler and more
consistent and significantly reduces the amount of constructor code in the
'thermophysicalModels' library.
* compressibleInterFoam
The creation of the 'viscosity' interface for the 'momentumTransport' models
allows the complex 'twoPhaseMixtureThermo' derived from 'rhoThermo' to be
replaced with the much simpler 'compressibleTwoPhaseMixture' derived from the
'viscosity' interface, avoiding the myriad of unused thermodynamic functions
required by 'rhoThermo' to be defined for the mixture.
Same for 'compressibleMultiphaseMixture' in 'compressibleMultiphaseInterFoam'.
This is a significant improvement in code and input consistency, simplifying
maintenance and further development as well as enhancing usability.
Henry G. Weller
CFD Direct Ltd.
The FOAM file format has not changed from version 2.0 in many years and so there
is no longer a need for the 'version' entry in the FoamFile header to be
required and to reduce unnecessary clutter it is now optional, defaulting to the
current file format 2.0.
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.
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.
