compressibleVoF supports cavitation fvModels which provide a more physical and
controllable approach to cavitation modelling than the simple homogeneous
equilibrium approximation used in cavitatingFoam.
The tutorials/multiphase/cavitatingFoam/RAS/throttle case has been converted to
tutorials/modules/compressibleVoF/throttle which demonstrates how to update
cases from cavitatingFoam to compressibleVoF.
A cavitatingFoam script is provided to redirect users to update their cases to
compressibleVoF.
to provide the old-time absolute flux. This avoids possible
pressure-velocity-flux decoupling (staggering) within the MRF region using
ddtCorr to better couple the velocity and flux fields.
Solver modules have replaced code that was previously shared between
solvers by means of #include-ing header files. Some of these headers are
now unused and have been removed. Others are only now used in a single
solver and have been moved into that solver.
executed with foamRun for single region simulations of foamMultiRun for
multi-region simulations. Replaces compressibleMultiphaseInterFoam and all the
corresponding tutorials have been updated and moved to
tutorials/modules/compressibleMultiphaseVoF.
compressibleMultiphaseVoF is derived from the multiphaseVoFSolver which adds
compressible multiphase capability to the VoFSolver base-class used as the basis
of all two-phase and multiphase VoF solvers.
Class
Foam::solvers::compressibleMultiphaseVoF
Description
Solver module for the solution of multiple compressible, 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.
A mixture approach for momentum transport is provided in which a single
laminar, RAS or LES model is selected to model the momentum stress.
Uses the flexible PIMPLE (PISO-SIMPLE) solution for time-resolved and
pseudo-transient and steady simulations.
SourceFiles
compressibleMultiphaseVoF.C
See also
Foam::solvers::VoFSolver
Foam::solvers::multiphaseVoFSolver
executed with foamRun for single region simulations of foamMultiRun for
multi-region simulations. Replaces multiphaseInterFoam and all the
corresponding tutorials have been updated and moved to
tutorials/modules/incompressibleMultiphaseVoF.
incompressibleMultiphaseVoF is derived from the multiphaseVoFSolver which adds
multiphase capability to the VoFSolver base-class used as the basis of all
two-phase and multiphase VoF solvers.
Class
Foam::solvers::incompressibleMultiphaseVoF
Description
Solver module for the solution of multiple 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.
A mixture approach for momentum transport is provided in which a single
laminar, RAS or LES model is selected to model the momentum stress.
Uses the flexible PIMPLE (PISO-SIMPLE) solution for time-resolved and
pseudo-transient and steady simulations.
SourceFiles
incompressibleMultiphaseVoF.C
See also
Foam::solvers::VoFSolver
Foam::solvers::multiphaseVoFSolver
used in the incompressibleMultiphaseMixture and compressibleMultiphaseMixture
respectively which are used in multiphaseInterFoam and
compressibleMultiphaseInterFoam respectively.
Also the PtrDictionary of phases has been replaced by PtrListDictionary of
phases and iterations over the linked-list replaced by forAll loops which is
easier to use and consistent with the multiphaseEuler solver module.
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.
Some momentumTransportModels like the laminar Stokes and generalisedNewtonian
models do no solve transport equations and the transport coefficients they
provide can be predicted at the beginning of the time-step rather than corrected
at the end, after conservative fluxes are available. A particular advantage of
this approach is that complex data cached in the momentumTransportModels
can now be deleted following mesh topology changes and recreated in the
predict() call which is more efficient than attempting to register and map the
data.
Currently the predict() function is only used for the Stokes and
generalisedNewtonian models but it will be extended in the future to cover many
LES models which also do not require the solution of transport equations.
All solvers and solver modules have been update to call the
momentumTransportModel::predict() function at the beginning of the time-step,
controlled by the new PIMPLE transportPredictionFirst control as appropriate.
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.
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.
Simulating the mixing of two miscible liquids is possible my considering
them as different species of a multicomponent fluid. This approach also
supports an arbitrary number of liquids. The twoLiquidMixingFoam solver
has therefore been removed and its tutorials converted to use the
multicomponentFluid solver module.
Now that thermal transport is implemented as an energy implicit correction on an
explicit temperature gradient formulation it is more efficient if the implicit
correction contains only the implicit terms of the matrix and not the explicit
non-orthogonal or anisotropic correction terms which are cancelled anyway when
the evaluation of the matrix for the current state is subtracted. The new
fvm::laplacianCorrection functions provide a convenient mechanism to efficiently
evaluate only the implicit correction to the laplacian and is now used in all
the thermophysicalTransportModels.
The thermodynamic density field is now named "rho" by default and only renamed
"thermo:rho" by solvers that create and maintain a separate continuity density
field which is named "rho". This change significantly simplifies and
standardises the specification of schemes and boundary conditions requiring
density as it is now always named "rho" or "rho.<phase>" unless under some very
unusual circumstances the thermodynamic rather than continuity density is
required for a solver maintaining both.
The advantage of this change is particularly noticeable for multiphase
simulations in which each phase has its own density now named "rho.<phase>"
rather than "thermo:rho.<phase>" as separate phase continuity density fields are
not required so for multiphaseEulerFoam the scheme specification:
"div\(alphaRhoPhi.*,\(p\|thermo:rho.*\)\)" Gauss limitedLinear 1;
is now written:
"div\(alphaRhoPhi.*,\(p\|rho.*\)\)" Gauss limitedLinear 1;
The basic thermophysical properties are now considered fundamental and complex
models like kineticTheoryModel using these names for some other purpose must
disambiguate using typedName to prepend the model name to the field name.
This change standardises, rationalises and simplifies the specification of
fvSchemes and boundary conditions.
thermo:rho will also be renamed rho in a subsequent commit to complete this
rationalisation.
the new fluidThermophysicalTransportModel and solidThermophysicalTransportModel
are derived from thermophysicalTransportModel providing a consistent and unified
interface for heat transport within and between regions. Coupled and external
heat-transfer boundary conditions can now be written independent of the
thermophysical properties or transport modelling of the regions providing
greater flexibility, simpler code and reduces the maintenance overhead.
The previous fluidThermophysicalTransportModel typedef has been renamed
fluidThermoThermophysicalTransportModel as it is instantiated on fluidThermo,
freeing the name fluidThermophysicalTransportModel for the new base-class.
so that derived classes can call the dictionary constructor without reading the
refValue, refGradient or valueFraction entries. This ensures that the
fvPatchField dictionary constructor is called, setting optional entries like
'libs' as required.
to handle isotropic and anisotropic is a consistent, general and extensible
manner, replacing the horrible hacks which were in solidThermo.
This is entirely consistent with thermophysicalTransportModel for fluids and
provides the q() and divq() for the solid energy conservation equations. The
transport model and properties are specified in the optional
thermophysicalTransport dictionary, the default model being isotropic if this
dictionary file is not present, thus providing complete backward-compatibility
for the common isotropic cases.
Anisotropic thermal conductivity is now handled in a much more general manner by
the anisotropic model:
Class
Foam::solidThermophysicalTransportModels::anisotropic
Description
Solid thermophysical transport model for anisotropic thermal conductivity
The anisotropic thermal conductivity field is evaluated from the solid
material anisotropic kappa specified in the physicalProperties dictionary
transformed into the global coordinate system using default
coordinate system and optionally additional coordinate systems specified
per-zone in the thermophysicalProperties dictionary.
Usage
Example of the anisotropic thermal conductivity specification in
thermophysicalProperties with two zone-based coordinate systems in
addition to the default:
\verbatim
model anisotropic;
// Default coordinate system
coordinateSystem
{
type cartesian;
origin (0 0 0);
coordinateRotation
{
type cylindrical;
e3 (1 0 0);
}
}
// Optional zone coordinate systems
zones
{
coil1
{
type cartesian;
origin (0.1 0.2 0.7);
coordinateRotation
{
type cylindrical;
e3 (0.5 0.866 0);
}
}
coil2
{
type cartesian;
origin (0.4 0.5 1);
coordinateRotation
{
type cylindrical;
e3 (0.866 0.5 0);
}
}
}
\endverbatim
This development required substantial rationalisation of solidThermo,
coordinateSystems and updates to the solid solver module, solidDisplacementFoam,
the wallHeatFlux functionObject, thermalBaffle and all coupled thermal boundary
conditions.
so that it can now be used with either the isothermalFluid or fluid solver
modules, thus supporting non-uniform fluid properties, compressibility and
thermal effect. This development makes the special potentialFreeSurfaceFoam
solver redundant as both the isothermalFluid and fluid solver modules are more
general and has been removed and replaced with a user redirection script.
The tutorials/multiphase/potentialFreeSurfaceFoam cases have been updated to run
with the isothermalFluid solver module:
tutorials/multiphase/potentialFreeSurfaceFoam/oscillatingBox
tutorials/multiphase/potentialFreeSurfaceFoam/movingOscillatingBox
which demonstrate how to upgrade potentialFreeSurfaceFoam cases to
isothermalFluid.
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.
Corrects granular phase heat transfer in cases where eddy diffusivity based
thermophysical transport models are used.
Patch contributed by VTT Technical Research Centre of Finland.
This completes the separation between thermodynamics and thermophysical
transport modelling and all models and boundary conditions involving heat
transfer now obtain the transport coefficients from the appropriate
ThermophysicalTransportModels rather than from fluidThermo.
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.
Population balance models now own their mass transfer rates, rather than
taking a non-constant reference to rates held by the phase system. This
means that they cannot reset or modify rates that relate to other
population balances.
MRF (multiple reference frames) can now be used to simulate SRF (single
reference frame) cases by defining the MRF zone to include all the cells is the
mesh and applying appropriate boundary conditions. The huge advantage of this
is that MRF can easily be added to any solver by the addition of forcing terms
in the momentum equation and absolute velocity to relative flux conversions in
the formulation of the pressure equation rather than having to reformulate the
momentum and pressure system based on the relative velocity as in traditional
SRF. Also most of the OpenFOAM solver applications and all the solver modules
already support MRF.
To enable this generalisation of MRF the transformations necessary on the
velocity boundary conditions in the MRF zone can no longer be handled by the
MRFZone class itself but special adapted fvPatchFields are required. Although
this adds to the case setup it provides much greater flexibility and now complex
inlet/outlet conditions can be applied within the MRF zone, necessary for some
SRF case and which was not possible in the original MRF implementation. Now for
walls rotating within the MRF zone the new 'MRFnoSlip' velocity boundary
conditions must be applied, e.g. in the
tutorials/modules/incompressibleFluid/mixerVessel2DMRF/constant/MRFProperties
case:
boundaryField
{
rotor
{
type MRFnoSlip;
}
stator
{
type noSlip;
}
front
{
type empty;
}
back
{
type empty;
}
}
similarly for SRF cases, e.g. in the
tutorials/modules/incompressibleFluid/mixerSRF case:
boundaryField
{
inlet
{
type fixedValue;
value uniform (0 0 -10);
}
outlet
{
type pressureInletOutletVelocity;
value $internalField;
}
rotor
{
type MRFnoSlip;
}
outerWall
{
type noSlip;
}
cyclic_half0
{
type cyclic;
}
cyclic_half1
{
type cyclic;
}
}
For SRF case all the cells should be selected in the MRFproperties dictionary
which is achieved by simply setting the optional 'selectionMode' entry to all,
e.g.:
SRF
{
selectionMode all;
origin (0 0 0);
axis (0 0 1);
rpm 1000;
}
In the above the rotational speed is set in RPM rather than rad/s simply by
setting the 'rpm' entry rather than 'omega'.
The tutorials/modules/incompressibleFluid/rotor2DSRF case is more complex and
demonstrates a transient SRF simulation of a rotor requiring the free-stream
velocity to rotate around the apparently stationary rotor which is achieved
using the new 'MRFFreestreamVelocity' velocity boundary condition. The
equivalent simulation can be achieved by simply rotating the entire mesh and
keeping the free-stream flow stationary and this is demonstrated in the
tutorials/modules/incompressibleFluid/rotor2DRotating case for comparison.
The special SRFSimpleFoam and SRFPimpleFoam solvers are now redundant and have
been replaced by redirection scripts providing details of the case migration
process.
to avoid name clash with the VoF surfaceTensionModels when both the
multiphaseEulerFoam and compressibleInterFoam libraries are linked into a single
executable.
