The old fluid-specific rhoThermo has been split into a non-fluid
specific part which is still called rhoThermo, and a fluid-specific part
called rhoFluidThermo. The rhoThermo interface has been added to the
solidThermo model. This permits models and solvers that access the
density to operate on both solid and fluid thermophysical models.
Mixture classes (e.g., pureMixtrure, coefficientMulticomponentMixture),
now have no fvMesh or volScalarField dependence. They operate on
primitive values only. All the fvMesh-dependent functionality has been
moved into the base thermodynamic classes. The 'composition()' access
function has been removed from multi-component thermo models. Functions
that were once provided by composition base classes such as
basicSpecieMixture and basicCombustionMixture are now implemented
directly in the relevant multi-component thermo base class.
in which the mass transfer rate is based on the theory of
evaporation/condensation on a plane interface.
Class
Foam::compressible::cavitationModels::Saito
Description
Saito cavitation model.
Reference:
\verbatim
Saito, Y., Takami, R., Nakamori, I., & Ikohagi, T. (2007).
Numerical analysis of unsteady behavior of cloud cavitation
around a NACA0015 foil. Computational Mechanics, 40, 85-96.
\endverbatim
Usage:
\table
Property | Description | Required | Default value
liquid | Name of the liquid phase | yes |
pSat | Saturation vapor pressure | yes |
Ca | Interfacial area concentration coefficient [1/m] | yes |
Cv | Vapourisation rate coefficient | yes |
Cc | Condensation rate coefficient | yes |
alphaNuc | Nucleation site volume fraction | yes |
\endtable
Example:
\verbatim
model Saito;
liquid liquid;
pSat 79995;
Ca 0.1; // Interfacial area concentration coefficient [1/m]
Cc 1;
Cv 1;
alphaNuc 0.01;
\endverbatim
SourceFiles
Saito.C
The filmCloudTransfer fvModel now supports an optional ejection model which
provides transfer of film to cloud by dripping from an inverted surface or
curvature separation:
Class
Foam::filmEjectionModels::dripping
Description
Dripping film to cloud ejection transfer model
On an inverted surface if the film thickness is sufficient to generate a
valid parcel the equivalent mass is removed from the film and transfered to
the cloud as a parcel containing droplets with a diameter obtained from
the specified parcelDistribution.
Usage
Example usage:
\verbatim
filmCloudTransfer
{
type filmCloudTransfer;
libs ("libfilmCloudTransfer.so");
ejection
{
model dripping;
deltaStable 5e-4;
minParticlesPerParcel 10;
parcelDistribution
{
type RosinRammler;
Q 0;
min 1e-3;
max 2e-3;
d 7.5e-05;
n 0.5;
}
}
}
\endverbatim
Class
Foam::filmEjectionModels::BrunDripping
Description
Brun dripping film to cloud ejection transfer model
If the film thickness exceeds the critical value needed to generate one or
more drops, the equivalent mass is removed from the film. The critical film
thickness is calculated from the Rayleigh-Taylor stability analysis of film
flow on an inclined plane by Brun et.al.
Reference:
\verbatim
Brun, P. T., Damiano, A., Rieu, P., Balestra, G., & Gallaire, F. (2015).
Rayleigh-Taylor instability under an inclined plane.
Physics of Fluids (1994-present), 27(8), 084107.
\endverbatim
The diameter of the drops formed are obtained from the local capillary
length multiplied by the \c dCoeff coefficient which defaults to 3.3.
Reference:
\verbatim
Lefebvre, A. (1988).
Atomisation and sprays
(Vol. 1040, No. 2756). CRC press.
\endverbatim
Usage
Example usage:
\verbatim
filmCloudTransfer
{
type filmCloudTransfer;
libs ("libfilmCloudTransfer.so");
ejection
{
model BrunDripping;
deltaStable 5e-4;
}
}
\endverbatim
Class
Foam::filmEjectionModels::curvatureSeparation
Description
Curvature induced separation film to cloud ejection transfer model
Assesses film curvature via the mesh geometry and calculates a force
balance of the form:
F_sum = F_inertial + F_body + F_surface_tension
If F_sum < 0, the film separates and is transferred to the cloud
if F_sum >= 0 the film remains attached.
Reference:
\verbatim
Owen, I., & Ryley, D. J. (1985).
The flow of thin liquid films around corners.
International journal of multiphase flow, 11(1), 51-62.
\endverbatim
Usage
Example usage:
\verbatim
filmCloudTransfer
{
type filmCloudTransfer;
libs ("libfilmCloudTransfer.so");
ejection
{
model curvatureSeparation;
deltaStable 5e-4;
}
}
\endverbatim
The new tutorials/modules/multiRegion/film/cylinderDripping tutorial case
demonstrates a film dripping into the cloud. The standard cylinder case is
turned upside-down (by changing the orientation of gravity) with an initial
0.2mm film of water over the surface which drips when the thickness is greater
than 0.5mm. Settings for all three ejection models are provided in the
constant/film/fvModels dictionary with the standard dripping model selected.
The two-phase VoF alphaContactAngleFvPatchScalarField class has been renamed
contactAngleFvPatchScalarField to avoid a name clash with the multiphaseEuler
version of alphaContactAngleFvPatchScalarField so that both VoF and
multiphaseEuler solver modules may be used in different regions of a
foamMultiRun simulation.
used in the alphaContactAngleFvPatchScalarField boundary condition to replace
the need to derive specialised versions for different contact angle evaluation
methods. This simplifies the code and provides a reusable system which could be
applied to other multiphase contact angle boundary conditions.
The patch field 'autoMap' and 'rmap' functions have been replaced with a
single 'map' function that can used to do any form of in-place
patch-to-patch mapping. The exact form of mapping is now controlled
entirely by the mapper object.
An example 'map' function is shown below:
void nutkRoughWallFunctionFvPatchScalarField::map
(
const fvPatchScalarField& ptf,
const fvPatchFieldMapper& mapper
)
{
nutkWallFunctionFvPatchScalarField::map(ptf, mapper);
const nutkRoughWallFunctionFvPatchScalarField& nrwfpsf =
refCast<const nutkRoughWallFunctionFvPatchScalarField>(ptf);
mapper(Ks_, nrwfpsf.Ks_);
mapper(Cs_, nrwfpsf.Cs_);
}
This single function replaces these two previous functions:
void nutkRoughWallFunctionFvPatchScalarField::autoMap
(
const fvPatchFieldMapper& m
)
{
nutkWallFunctionFvPatchScalarField::autoMap(m);
m(Ks_, Ks_);
m(Cs_, Cs_);
}
void nutkRoughWallFunctionFvPatchScalarField::rmap
(
const fvPatchScalarField& ptf,
const labelList& addr
)
{
nutkWallFunctionFvPatchScalarField::rmap(ptf, addr);
const nutkRoughWallFunctionFvPatchScalarField& nrwfpsf =
refCast<const nutkRoughWallFunctionFvPatchScalarField>(ptf);
Ks_.rmap(nrwfpsf.Ks_, addr);
Cs_.rmap(nrwfpsf.Cs_, addr);
}
Calls to 'autoMap' should be replaced with calls to 'map' with the same
mapper object and the patch field itself provided as the source. Calls
to 'rmap' should be replaced with calls to 'map' by wrapping the
addressing in a 'reverseFvPatchFieldMapper' (or
'reversePointPatchFieldMapper') object.
This change simplifies the creation of new patch fields and hence
improves extensibility. It also provides more options regarding general
mapping strategies between patches. Previously, general abstracted
mapping was only possible in 'autoMap'; i.e., from a patch to itself.
Now, general mapping is possible between different patches.
executed with foamRun for single region simulations of foamMultiRun for
multi-region simulations. Replaces interFoam and all the corresponding
tutorials have been updated and moved to tutorials/modules/incompressibleVoF.
Both incompressibleVoF and compressibleVoF solver modules are derived from the
common two-phase VoF base-class solvers::VoFSolver which handles the
complexities of VoF interface-compression, boundedness and conservation with
2nd-order schemes in space and time using the semi-implicit MULES limiter and
solution proceedure. This maximises code re-use, improves readability and
simplifies maintenance.
Class
Foam::solvers::incompressibleVoF
Description
Solver module for for 2 incompressible, isothermal immiscible fluids using a
VOF (volume of fluid) phase-fraction based interface capturing approach,
with optional mesh motion and mesh topology changes including adaptive
re-meshing.
The momentum and other fluid properties are of the "mixture" and a single
momentum equation is solved.
Either mixture or two-phase transport modelling may be selected. In the
mixture approach a single laminar, RAS or LES model is selected to model the
momentum stress. In the Euler-Euler two-phase approach separate laminar,
RAS or LES selected models are selected for each of the phases.
Uses the flexible PIMPLE (PISO-SIMPLE) solution for time-resolved and
pseudo-transient and steady simulations.
Optional fvModels and fvConstraints are provided to enhance the simulation
in many ways including adding various sources, Lagrangian
particles, surface film etc. and constraining or limiting the solution.
SourceFiles
incompressibleVoF.C
See also
Foam::solvers::VoFSolver
Foam::solvers::compressibleVoF
In order to ensure temperature consistency between the phases it is necessary to
solve for the mixture temperature rather than the mixture energy or phase
energies which makes it very difficult to conserve energy. The new temperature
equation is a temperature correction on the combined phase energy equations
which will conserve the phase and mixture energies at convergence. The
heat-flux (Laplacian) term is maintained in mixture temperature form so
heat-transfer boundary conditions, in particular for CHT, remain in terms of the
mixture kappaEff. The fvModels are applied to the phase energy equations and
the implicit part converted into an implicit term in the temperature correction
part of the equation to improve convergence and stability.
This development has required some change to the alphaEqn.H and interFoam has
been updated for consistency in preparation for conversion into the
solvers::incompressibleVoF modular module.
All compressibleVoF fvModels and tutorial cases have been updated for the above
change. Note that two entries are now required for the convection terms in the
temperature equation, one for explicit phase energy terms and another for the
implicit phase temperature correction terms, e.g.
tutorials/modules/compressibleVoF/ballValve
div(alphaRhoPhi,e) Gauss limitedLinear 1;
div(alphaRhoPhi,T) Gauss upwind;
In the above the upwind scheme is selected for the phase temperature correction
terms as they are corrections and will converge to a zero contribution. However
there may be cases which converge better if the same scheme is used for both the
energy and temperature terms, more testing is required.
The timeName() function simply returns the dimensionedScalar::name() which holds
the user-time name of the current time and now that timeName() is no longer
virtual the dimensionedScalar::name() can be called directly. The timeName()
function implementation is maintained for backward-compatibility.
This adds cavitation modelling to the multiphaseEuler solver module as a
phaseTransfer model. The underlying cavitation modelling is the same as
for the compressibleVoF module.
An example specification in constant/phaseProperties is shown below:
phaseTransfer
{
gas_liquid
{
type cavitation;
model Kunz;
liquid water;
pSat 80000;
UInf 5.33;
tInf 0.028142589;
Cc 100;
Cv 100;
}
}
Based on code contributed by Petteri Peltonen, VTT.
The cavitation models used by the compressibleVoF module can now have a
temperature-dependent saturation pressure model specified. For example,
in the constant/fvModels file of a compressibleVoF case:
VoFCavitation
{
type VoFCavitation;
libs ("libcompressibleVoFCavitation.so");
model SchnerrSauer;
liquid water;
// Constant saturation pressure
//pSat 2300;
// Antoine equation for temperature-dependent saturation pressure
pSat
{
type Antoine;
A 22;
B -3000;
C -500;
}
n 1.6e+13;
dNuc 2.0e-06;
Cc 1;
Cv 1;
}
The cavitation models used by the interFoam solver and the
compressibleVoF solver module can now be applied regardless of the
ordering of the liquid and vapour phases. A "liquid" keyword is now
required in the model specification in order to control which phase is
considered to be the condensed liquid state. Previously the liquid phase
was assumed to be the first of the two phases.
Replacing the specific twoPhaseChangeModel with a consistent and general fvModel
interface will support not just cavitation using the new compressible
VoFCavitation fvModel but also other phase-change and interface manipulation
models in the future and is easier to use for case-specific and other user
customisation.
Class
Foam::fv::compressible::VoFCavitation
Description
Cavitation fvModel
Usage
Example usage:
\verbatim
VoFCavitation
{
type VoFCavitation;
libs ("libcompressibleVoFCavitation.so");
model SchnerrSauer;
KunzCoeffs
{
pSat 2300; // Saturation pressure
UInf 20.0;
tInf 0.005; // L = 0.1 m
Cc 1000;
Cv 1000;
}
MerkleCoeffs
{
pSat 2300; // Saturation pressure
UInf 20.0;
tInf 0.005; // L = 0.1 m
Cc 80;
Cv 1e-03;
}
SchnerrSauerCoeffs
{
pSat 2300; // Saturation pressure
n 1.6e+13;
dNuc 2.0e-06;
Cc 1;
Cv 1;
}
}
\endverbatim
The cavitating ballValve tutorial has been updated to use the new VoFCavitation
fvModel.
Replacing the specific twoPhaseChangeModel with a consistent and general fvModel
interface will support not just cavitation using the new VoFCavitation fvModel
but also other phase-change and interface manipulation models in the future and
is easier to use for case-specific and other user customisation.
executed with foamRun for single region simulations of foamMultiRun for
multi-region simulations. Replaces compressibleInterFoam and all the
corresponding tutorials have been updated and moved to
tutorials/modules/compressibleVoF.
Class
Foam::solvers::compressibleVoF
Description
Solver module for for 2 compressible, non-isothermal immiscible fluids
using a VOF (volume of fluid) phase-fraction based interface capturing
approach, with optional mesh motion and mesh topology changes including
adaptive re-meshing.
The momentum and other fluid properties are of the "mixture" and a single
momentum equation is solved.
Either mixture or two-phase transport modelling may be selected. In the
mixture approach a single laminar, RAS or LES model is selected to model the
momentum stress. In the Euler-Euler two-phase approach separate laminar,
RAS or LES selected models are selected for each of the phases.
Uses the flexible PIMPLE (PISO-SIMPLE) solution for time-resolved and
pseudo-transient and steady simulations.
Optional fvModels and fvConstraints are provided to enhance the simulation
in many ways including adding various sources, Lagrangian
particles, surface film etc. and constraining or limiting the solution.
SourceFiles
compressibleVoF.C
See also
Foam::solvers::fluidSolver
The typedName functions prepend the typeName to the object/field name to make a
unique name within the context of model or type.
Within a type which includes a typeName the typedName function can be called
with just the name of the object, e.g. within the kEpsilon model
typeName("G")
generates the name
kEpsilon:G
To create a typed name within another context the type name can be obtained from
the type specified in the function instantiation, e.g.
Foam::typedName<viscosityModel>("nu")
generates the name
viscosityModel:nu
This supersedes the modelName functionality provided in IOobject which could
only be used for IOobjects which provide the typeName, whereas typedName can be
used for any type providing a typeName.
If the sequence of meshes are decomposed independently the number, order and
potentially type of processor patches is likely to change. Thus the processor
patches and patch fields must be replaced with those of the new mesh.
fvMesh is no longer derived from fvSchemes and fvSolution, these are now
demand-driven and accessed by the member functions schemes() and solution()
respectively. This means that the system/fvSchemes and system/fvSolution files
are no longer required during fvMesh constructions simplifying the mesh
generation and manipulation phase; theses files are read on the first call of
their access functions.
The fvSchemes member function names have also been simplified taking advantage
of the context in which they are called, for example
mesh.ddtScheme(fieldName) -> mesh.schemes().ddt(fieldName)
For some cases, in particular those with very small cells created by snapping in
corners for example, it may be beneficial to convergence rate to limit the
minimum LTS time-step, the new minDeltaT control provides this.
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
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.
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.
