Now that Cp and Cv are cached it is more convenient and consistent and slightly
more efficient to cache thermal conductivity kappa rather than thermal
diffusivity alpha which is not a fundamental property, the appropriate form
depending on the energy solved for. kappa is converted into the appropriate
thermal diffusivity for the energy form solved for by dividing by the
corresponding cached heat capacity when required, which is efficient.
Following the addition of the new moments functionObject, all related
functionality was removed from sizeDistribution.
In its revised version, sizeDistribution allows for different kinds of
weighted region averaging in case of field-dependent representative
particle properties.
A packaged function has also been added to allow for command line solver
post-processing.
For example, the following function object specification returns the
volume-based number density function:
numberDensity
{
type sizeDistribution;
libs ("libmultiphaseEulerFoamFunctionObjects.so");
writeControl writeTime;
populationBalance bubbles;
functionType numberDensity;
coordinateType volume;
setFormat raw;
}
The same can be achieved using a packaged function:
#includeFunc sizeDistribution
(
populationBalance=bubbles,
functionType=numberDensity,
coordinateType=volume,
funcName=numberDensity
)
Or on the command line:
multiphaseEulerFoam -postProcess -func "
sizeDistribution
(
populationBalance=bubbles,
functionType=numberDensity,
coordinateType=volume,
funcName=numberDensity
)"
Patch contributed by Institute of Fluid Dynamics,
Helmholtz-Zentrum Dresden - Rossendorf (HZDR)
This function calculates integral (integer moments) or mean properties
(mean, variance, standard deviation) of a size distribution computed with
multiphaseEulerFoam. It has to be run with multiphaseEulerFoam, either
at run-time or with -postProcess. It will not work with the postProcess
utility.
The following function object specification for example returns the first
moment of the volume-based number density function which is equivalent to
the phase fraction of the particulate phase:
moments
{
type moments;
libs ("libmultiphaseEulerFoamFunctionObjects.so");
executeControl timeStep;
writeControl writeTime;
populationBalance bubbles;
momentType integerMoment;
coordinateType volume;
order 1;
}
The same can be achieved using a packaged function:
#includeFunc moments
(
populationBalance=bubbles,
momentType=integerMoment,
coordinateType=volume,
order=1,
funcName=moments
)
Or on the command line:
multiphaseEulerFoam -postProcess -func "
moments
(
populationBalance=bubbles,
momentType=integerMoment,
coordinateType=volume,
order=1,
funcName=moments
)"
Patch contributed by Institute of Fluid Dynamics,
Helmholtz-Zentrum Dresden - Rossendorf (HZDR)
There is no longer any need for the surfaceFilmModel abstract base class and
"New" selection method as surface films are now handled within the fvModel
framework. This makes the surfaceFilmModel entry in the surfaceFilmProperties
dictionary redundant.
The surfaceFilm and VoFSurfaceFilm fvModels now instantiate a thermoSingleLayer
providing direct access to all the film functions, simplifying the
implementation better ensuring consistency between the film and primary region
equations.
These models are quite configuration specific. It makes sense to make
them sub-models of the force (drag or lift) models that use them, rather
than making them fundamental properties of the phase system.
Sampled sets and streamlines now write all their fields to the same
file. This prevents excessive duplication of the geometry and makes
post-processing tasks more convenient.
"axis" entries are now optional in sampled sets and streamlines. When
omitted, a default entry will be used, which is chosen appropriately for
the coordinate set and the write format. Some combinations are not
supported. For example, a scalar ("x", "y", "z" or "distance") axis
cannot be used to write in the vtk format, as vtk requires 3D locations
with which to associate data. Similarly, a point ("xyz") axis cannot be
used with the gnuplot format, as gnuplot needs a single scalar to
associate with the x-axis.
Streamlines can now write out fields of any type, not just scalars and
vectors, and there is no longer a strict requirement for velocity to be
one of the fields.
Streamlines now output to postProcessing/<functionName>/time/<file> in
the same way as other functions. The additional "sets" subdirectory has
been removed.
The raw set writer now aligns columns correctly.
The handling of segments in coordSet and sampledSet has been
fixed/completed. Segments mean that a coordinate set can represent a
number of contiguous lines, disconnected points, or some combination
thereof. This works in parallel; segments remain contiguous across
processor boundaries. Set writers now only need one write method, as the
previous "writeTracks" functionality is now handled by streamlines
providing the writer with the appropriate segment structure.
Coordinate sets and set writers now have a convenient programmatic
interface. To write a graph of A and B against some coordinate X, in
gnuplot format, we can call the following:
setWriter::New("gnuplot")->write
(
directoryName,
graphName,
coordSet(true, "X", X), // <-- "true" indicates a contiguous
"A", // line, "false" would mean
A, // disconnected points
"B",
B
);
This write function is variadic. It supports any number of
field-name-field pairs, and they can be of any primitive type.
Support for Jplot and Xmgrace formats has been removed. Raw, CSV,
Gnuplot, VTK and Ensight formats are all still available.
The old "graph" functionality has been removed from the code, with the
exception of the randomProcesses library and associated applications
(noise, DNSFoam and boxTurb). The intention is that these should also
eventually be converted to use the setWriters. For now, so that it is
clear that the "graph" functionality is not to be used elsewhere, it has
been moved into a subdirectory of the randomProcesses library.
MULES no longer synchronises the limiter field using syncTools. Surface
boundary field synchronisation is now done with a surface-field-specific
communication procedure that should result in scaling benefits relative
to syncTools. This change also means that the limiter does not need to
be continuous face field which is then sliced; it can be a standard
surface field.
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
With this change each functionObject provides the list of fields required so
that the postProcess utility can pre-load them before executing the list of
functionObjects. This provides a more convenient interface than using the
-field or -fields command-line options to postProcess which are now redundant.
replacing the virtual functions overridden in engineTime.
Now the userTime conversion function in Time is specified in system/controlDict
such that the solver as well as all pre- and post-processing tools also operate
correctly with the chosen user-time.
For example the user-time and rpm in the tutorials/combustion/XiEngineFoam/kivaTest case are
now specified in system/controlDict:
userTime
{
type engine;
rpm 1500;
}
The default specification is real-time:
userTime
{
type real;
}
but this entry can be omitted as the real-time class is instantiated
automatically if the userTime entry is not present in system/controlDict.
The temperature equation in compressibleInterFoam is derived from the phase
total internal energy equations including the kinetic energy source terms.
While this formulation handles pressure loss more accurately the kinetic energy
source terms can cause numerical problems and more likely to induce negative
temperatures in regions where the pressure drops rapidly. For such cases it may
be beneficial to solve a temperature equation derived from the phase internal
energy equations, i.e. without the kinetic energy source terms which is now
selectable by setting the optional totalInternalEnergy entry in
constant/phaseProperties to false:
totalInternalEnergy false;
When this entry is omitted the total energy form is used providing
backward-compatibility.
Mesh motion and topology change are now combinable run-time selectable options
within fvMesh, replacing the restrictive dynamicFvMesh which supported only
motion OR topology change.
All solvers which instantiated a dynamicFvMesh now instantiate an fvMesh which
reads the optional constant/dynamicFvMeshDict to construct an fvMeshMover and/or
an fvMeshTopoChanger. These two are specified within the optional mover and
topoChanger sub-dictionaries of dynamicFvMeshDict.
When the fvMesh is updated the fvMeshTopoChanger is first executed which can
change the mesh topology in anyway, adding or removing points as required, for
example for automatic mesh refinement/unrefinement, and all registered fields
are mapped onto the updated mesh. The fvMeshMover is then executed which moved
the points only and calculates the cell volume change and corresponding
mesh-fluxes for conservative moving mesh transport. If multiple topological
changes or movements are required these would be combined into special
fvMeshMovers and fvMeshTopoChangers which handle the processing of a list of
changes, e.g. solidBodyMotionFunctions:multiMotion.
The tutorials/multiphase/interFoam/laminar/sloshingTank3D3DoF case has been
updated to demonstrate this new functionality by combining solid-body motion
with mesh refinement/unrefinement:
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: dev
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
location "constant";
object dynamicMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
mover
{
type motionSolver;
libs ("libfvMeshMovers.so" "libfvMotionSolvers.so");
motionSolver solidBody;
solidBodyMotionFunction SDA;
CofG (0 0 0);
lamda 50;
rollAmax 0.2;
rollAmin 0.1;
heaveA 4;
swayA 2.4;
Q 2;
Tp 14;
Tpn 12;
dTi 0.06;
dTp -0.001;
}
topoChanger
{
type refiner;
libs ("libfvMeshTopoChangers.so");
// How often to refine
refineInterval 1;
// Field to be refinement on
field alpha.water;
// Refine field in between lower..upper
lowerRefineLevel 0.001;
upperRefineLevel 0.999;
// Have slower than 2:1 refinement
nBufferLayers 1;
// Refine cells only up to maxRefinement levels
maxRefinement 1;
// Stop refinement if maxCells reached
maxCells 200000;
// Flux field and corresponding velocity field. Fluxes on changed
// faces get recalculated by interpolating the velocity. Use 'none'
// on surfaceScalarFields that do not need to be reinterpolated.
correctFluxes
(
(phi none)
(nHatf none)
(rhoPhi none)
(alphaPhi.water none)
(meshPhi none)
(meshPhi_0 none)
(ghf none)
);
// Write the refinement level as a volScalarField
dumpLevel true;
}
// ************************************************************************* //
Note that currently this is the only working combination of mesh-motion with
topology change within the new framework and further development is required to
update the set of topology changers so that topology changes with mapping are
separated from the mesh-motion so that they can be combined with any of the
other movements or topology changes in any manner.
All of the solvers and tutorials have been updated to use the new form of
dynamicMeshDict but backward-compatibility was not practical due to the complete
reorganisation of the mesh change structure.
used to check the existence of and open an object file, read and check the
header without constructing the object.
'typeIOobject' operates in an equivalent and consistent manner to 'regIOobject'
but the type information is provided by the template argument rather than via
virtual functions for which the derived object would need to be constructed,
which is the case for 'regIOobject'.
'typeIOobject' replaces the previous separate functions 'typeHeaderOk' and
'typeFilePath' with a single consistent interface.
Provided for use with mixture turbulence models in interFoam and
compressibleInterFoam.
Class
Foam::fv::VoFTurbulenceDamping
Description
Free-surface turbulence damping function
Adds an extra source term to the mixture or phase epsilon or omega
equation to reduce turbulence generated near a free-surface. The
implementation is based on
Reference:
\verbatim
Frederix, E. M. A., Mathur, A., Dovizio, D., Geurts, B. J.,
& Komen, E. M. J. (2018).
Reynolds-averaged modeling of turbulence damping
near a large-scale interface in two-phase flow.
Nuclear engineering and design, 333, 122-130.
\endverbatim
but with an improved formulation for the coefficient \c A appropriate for
unstructured meshes including those with split-cell refinement patterns.
However the dimensioned length-scale coefficient \c delta remains and must
be set appropriatly for the case by performing test runs and comparing with
known results. Clearly this model is far from general and more research is
needed in order that \c delta can be obtained directly from the interface
flow and turbulence conditions.
Usage
Example usage:
\verbatim
VoFTurbulenceDamping
{
type VoFTurbulenceDamping;
libs ("libVoFTurbulenceDamping.so");
// Interface turbulence damping length scale
// This is a required input as described in section 3.3 of the paper
delta 1e-4;
// phase water; // Optional phase name
}
\endverbatim
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 writer class has been renamed setWriter in order to clarify its
usage. The coordSet and setWriter classes have been moved into the
sampling library, as this fits their usage.
to ensure that the contact angle specification is used irrespective of which
phase it is specified in. An error is reported if both phases of the interface
pair have a contact angle specification as the specifications might be
inconsistent.
Resolves bug-report https://bugs.openfoam.org/view.php?id=3688
to ensure that the contact angle specification is used irrespective of which
phase it is specified in. An error is reported if both phases of the interface
pair have a contact angle specification as the specifications might be
inconsistent.
Resolves bug-report https://bugs.openfoam.org/view.php?id=3688
The pressure work term for total internal energy is div(U p) which can be
discretised is various ways, given a mass flux field phi it seems logical to
implement it in the form div(phi/interpolate(rho), p) but this is not exactly
consistent with the relationship between enthalpy and internal energy (h = e +
p/rho) and the transport of enthalpy, it would be more consistent to implement
it in the form div(phi, p/rho). A further improvement in consistency can be
gained by using the same convection scheme for this work term and the convection
term div(phi, e) and for reacting solvers this is easily achieved by using the
multi-variate limiter mvConvection provided for energy and specie convection.
This more consistent total internal energy work term has now been implemented in
all the compressible and reacting flow solvers and provides more accurate
solutions when running with internal energy, particularly for variable density
mixing cases with small pressure variation.
For non-reacting compressible solvers this improvement requires a change to the
corresponding divScheme in fvSchemes:
"div\(alphaPhi.*,p\)" -> "div\(alphaRhoPhi.*,\(p\|thermo:rho.*\)\)"
and all the tutorials have been updated accordingly.
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)
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.
