Field algebra has been optimised by careful ordering to minimise the
number of expensive operations; e.g., changing a/b/c to a/(b*c) in order
to minimise the number of divisions.
Some minor consistency improvements have also been made throughout
population balance.
Patch contributed by Institute of Fluid Dynamics,
Helmholtz-Zentrum Dresden - Rossendorf (HZDR)
A phase system has been added that combines interface composition phase
change modelling and population balance modelling. It can be selected in
constant/phaseProperties using the following setting:
type interfaceCompositionPhaseChangePopulationBalanceMultiphaseSystem;
In order to facilitate the operation of population balance models with
mass transfers generated by the interface composition system, the full
interfacial mass transfer rate is now being stored, as well as the
linearised specie transfers. This means the mass transfer rates
associated with the interface composition mechanism can be looked up and
utilised by sub models.
Based on a patch contributed by Institute of Fluid Dynamics,
Helmholtz-Zentrum Dresden - Rossendorf (HZDR)
for buoyant solvers buoyantPimpleFoam, buoyantSimpleFoam and
buoyantReactingFoam:
Class
Foam::hydrostaticInitialisation
Description
Optional hydrostatic initialisation of p_rgh and p by solving for and
caching the hydrostatic ph_rgh and updating the density such that
p = ph_rgh + rho*gh + pRef
This initialisation process is applied at the beginning of the run (not on
restart) if the \c hydrostaticInitialisation switch is set true in
fvSolution/PIMPLE or fvSolution/SIMPLE. The calculation is iterative if the
density is a function of pressure and an optional number of iterations \c
nHydrostaticCorrectors may be specified which defaults to 5.
The fireFoam solver has solver has been replaced by the more general
buoyantReactingFoam solver, which supports buoyant compressible reacting flow
coupled to multiple run-time-selectable lagrangian clouds and surface film
modelling and optional hydrostatic initialisation of the pressure and p_rgh.
Hydrostatic initialisation of the pressure fields is useful for large fires in
open domains where the stability of the initial flow is dominated by the initial
pressure distribution in the domain and at the boundaries. The optional
hydrostaticInitialization switch in fvSolution/PIMPLE with
nHydrostaticCorrectors enables hydrostatic initialisation, e.g.
PIMPLE
{
momentumPredictor yes;
nOuterCorrectors 1;
nCorrectors 2;
nNonOrthogonalCorrectors 0;
hydrostaticInitialization yes;
nHydrostaticCorrectors 5;
}
and the resulting ph_rgh field can be used with the prghTotalHydrostaticPressure
p_rgh boundary condition to apply this hydrostatic pressure distribution at the
boundaries throughout the simulation.
See the following cases for examples transferred from fireFoam:
$FOAM_TUTORIALS/combustion/buoyantReactingFoam/RAS
With the new fvModels framework it is now possible to implement complex models
and wrappers around existing complex models which can then be optionally
selected in any general solver which provides compatible fields and
thermophysical properties. This simplifies code development and maintenance by
significantly reducing complex code duplication and also provide the opportunity
of running these models in other solvers without the need for code duplication
and alteration.
The immediate advantage of this development is the replacement of the
specialised Lagrangian solvers with their general counterparts:
reactingParticleFoam -> reactingFoam
reactingParcelFoam -> reactingFoam
sprayFoam -> reactingFoam
simpleReactingParticleFoam -> reactingFoam
buoyantReactingParticleFoam -> buoyantReactingFoam
For example to run a reactingParticleFoam case in reactingFoam add the following
entries in constant/fvModels:
buoyancyForce
{
type buoyancyForce;
}
clouds
{
type clouds;
libs ("liblagrangianParcel.so");
}
which add the acceleration due to gravity needed by Lagrangian clouds and the
clouds themselves.
See the following cases for examples converted from reactingParticleFoam:
$FOAM_TUTORIALS/combustion/reactingFoam/Lagrangian
and to run a buoyantReactingParticleFoam case in buoyantReactingFoam add the
following entry constant/fvModels:
clouds
{
type clouds;
libs ("liblagrangianParcel.so");
}
to add support for Lagrangian clouds and/or
surfaceFilm
{
type surfaceFilm;
libs ("libsurfaceFilmModels.so");
}
to add support for surface film. The buoyancyForce fvModel is not required in
this case as the buoyantReactingFoam solver has built-in support for buoyancy
utilising the p_rgh formulation to provide better numerical handling for this
force for strongly buoyancy-driven flows.
See the following cases for examples converted from buoyantReactingParticleFoam:
$FOAM_TUTORIALS/combustion/buoyantReactingFoam/Lagrangian
All the tutorial cases for the redundant solvers have been updated and converted
into their new equivalents and redirection scripts replace these solvers to
provide users with prompts on which solvers have been replaced by which and
information on how to upgrade their cases.
To support this change and allow all previous Lagrangian tutorials to run as
before the special Lagrangian solver fvSolution/PIMPLE control
solvePrimaryRegion has been replaced by the more general and useful controls:
models : Enable the fvModels
thermophysics : Enable thermophysics (energy and optional composition)
flow : Enable flow (pressure/velocity system)
which also replace the fvSolution/PIMPLE control frozenFlow present in some
solvers. These three controls can be used in various combinations to allow for
example only the fvModels to be evaluated, e.g. in
$FOAM_TUTORIALS/combustion/buoyantReactingFoam/Lagrangian/rivuletPanel
PIMPLE
{
models yes;
thermophysics no;
flow no;
.
.
.
so that only the film is solved. Or during the start-up of a case it might be
beneficial to run the pressure-velocity system for a while without updating
temperature which can be achieved by switching-off thermophysics. Also the
behaviour of the previous frozenFlow switch can be reproduced by switching flow
off with the other two switches on, allowing for example reactions, temperature
and composition update without flow.
for consistency with the handling of restarts in Time. See
commit 7aca9bfa78
Author: Henry Weller <http://cfd.direct>
Date: Fri Dec 11 13:37:16 2020 +0000
Time: Added beginTime used to rationalise the write times when restarting
Now if a case is restarted from an arbitrary time, for example one generated at
a premature stop condition, or with an increased writeInterval, the subsequent
time directories written are referenced to the original start time of the case
rather than the restart time.
The themo tables used in wallBoiling have had their Cp/Cv values
corrected, and have been coarsened and reduced in size to bound only the
operating point of the wallBoiling tutorials. They have also been moved
to $FOAM_TUTORIALS/resources/thermoData.
The correction to thermophysical properties has improved the stability
of these cases. As a result it has been possible to reduce the amount of
under-relaxation used in the wall modelling.
The phase-fraction filtering of the compressibility terms is present to avoid
spurious phase-change due to numerical noise. The fvModels contribution may
cause physical phase-change due to cavitation, boiling, transfer from film or
VoF even where none of the phase is present and hence must be added after the
compressibility filtering.
With VoFClouds and VoFSurfaceFilm compressibleInterFoam supports Lagrangian
clouds which can impinge on walls forming a film which in turn can transfer to
the VoF when the film is thick enough to resolve. The new tutorial case
tutorials/multiphase/compressibleInterFoam/laminar/cylinder
is provided to demonstrate this functionality.
Direct transfer of droplets to the VoF phase is not yet supported but will be
added later.
A cloud may now contain species that do not exist within the carrier
thermodynamics. Correspondence between lagrangian and carrier components
is only required when there is phase change.
The thermo parcel now supports thermophysical property modelling. This
particle does not store phase or specie fractions so it only provides a
single phase with a uniform composition. Additional specification is
required in the cloud subModel configuration in order to select the
specie. For example:
compositionModel singlePhaseMixture;
singlePhaseMixtureCoeffs
{
phases
(
solid
{
CaCO3 1;
}
);
}
The reduced SLGThermo has been renamed parcelThermo to better represent the
purpose.
parcelThermo is not created and stored in the cloud that requires it rather than
requiring it to be created in the solver createFields and passed to the cloud on
construction.
This makes usage of transformPoints the same as for
surfaceTransformPoints. Transformations are supplied as a string and are
applied in sequence.
Usage
transformPoints "\<transformations\>" [OPTION]
Supported transformations:
- "translate=<translation vector>"
Translational transformation by given vector
- "rotate=(<n1 vector> <n2 vector>)"
Rotational transformation from unit vector n1 to n2
- "Rx=<angle [deg] about x-axis>"
Rotational transformation by given angle about x-axis
- "Ry=<angle [deg] about y-axis>"
Rotational transformation by given angle about y-axis
- "Rz=<angle [deg] about z-axis>"
Rotational transformation by given angle about z-axis
- "Ra=<axis vector> <angle [deg] about axis>"
Rotational transformation by given angle about given axis
- "scale=<x-y-z scaling vector>"
Anisotropic scaling by the given vector in the x, y, z
coordinate directions
Example usage:
transformPoints \
"translate=(-0.05 -0.05 0), \
Rz=45, \
translate=(0.05 0.05 0)"
