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.
Lagrangian injections now have a 'uniformParcelSize' control, which
specifies what size of the parcels is kept uniform during a given time
step. This control can be set to 'nParticles', 'surfaceArea' or
'volume'. The particle sizes, by contrast, are specified by the size
distribution.
For example, if 'uniformParcelSize nParticles;' is specified then all
parcels introduced at a given time will have the same number of
particles. Every particle in a parcel has the same properties, including
diameter. So, in this configuration, the larger diameter parcels contain
a much larger fraction of the total particulate volume than the smaller
diameter ones. This may be undesirable as the effect of a parcel on the
simulation might be more in proportion with its volume than with the
number of particles it represents. It might be preferable to create a
greater proportion of large diameter parcels so that their more
significant effect is represented by a finer Lagrangian discretisation.
This can be achieved by setting 'uniformParcelSize volume;'. A setting
of 'uniformParcelSize surfaceArea;' might be appropriate if the limiting
effect of a Lagrangian element scales with its surface area; interfacial
evaporation, for example.
Previously, this control was provided by 'parcelBasisType'. However,
this control also effectively specified the size exponent of the
supplied distribution. This interdependence was not documented and was
problematic in that it coupled physical and numerical controls.
'parcelBasisType' has been removed, and the size exponent of the
distribution is now specified independently of the new
'uniformParcelSize' control along with the rest of the distribution
coefficients or data. See the previous commit for details.
It is still possible to specify a fixed number of particles per parcel
using the 'nParticle' control. The presence of this control is used to
determine whether or not the number of particles per parcel is fixed, so
a 'fixed' basis type is no longer needed.
A number of bugs have been fixed with regards to lack of
interoperability between the various settings in the injection models.
'uniformParcelSize' can be changed freely and the number of parcels and
amount of mass that an injector introduces will not change (this was not
true of 'parcelBasisType'). Redundant settings are no longer read by the
injection models; e.g., mass is not read if the number of particles per
parcel is fixed, duration is not specified for steady tracking, etc...
The 'inflationInjection' model has been removed as there are no examples
of its usage, its purpose was not clearly documented, and it was not
obvious how it should be updated as a result of these changes.
The calculation of the diffusion number has been put into a form
consistent with finite-volume, rather than the finite-difference form
that was used previously.
This difference in formulations is analogus to that of the Courant
number in the fluid solvers. Whilst a textbook will typically define the
courant number as equal to 'U*deltaT/deltaX', in a finite-volume context
it is more appropriate to define it as 'Sum(phi)/V*deltaT' (where 'Sum'
is a sum over the cell's faces). Similarly, the finite-difference
Fourier number, 'kappa/rho/Cp*deltaT/deltaX^2', is more consistently
expressed for finite-volume as 'Sum(Sf*kappa*deltaX)/(V*rho*Cp)*deltaT'.
This makes the calculation of the diffusion number less sensitive to the
presence of small, poor quality faces, and therefore makes time-step
adjustment more robust on arbitrary polyhedral meshes.
This completes commit 381e0921 and permits patches on the "top" of
extruded regions to determine the point locations opposite as well as
the face centres and areas. This means that patches with dissimilar
meshes can now be coupled via the patchToPatch interpolation engine.
A few fixes have also been applied to extrudeToRegionMesh to make the
intrude option compatibile with extrusion into internal faces and
between opposing zones/sets/patches. The 'shadow' entries used for
extrusion inbetween opposing zones/sets/patches have also been renamed
to 'opposite' for consistency with the patch names and patch types
entries; e.g.,
faceZones (fz1 fz3);
oppositeFaceZones (fz2 fz4); // <-- was 'faceZonesShadow'
faceSets (fs1 fs3);
oppositeFaceSets (fs2 fs4); // <-- was 'faceSetsShadow'
patches (p1 p3);
oppositePatches (p2 p4); // <-- was 'patchesShadow'
The parcel transfer occurs from the cloudFilmTransfer surfaceFilmModel specified
in the <fluid> region constant/<fluid>/cloudProperties dictionary:
.
.
.
libs ("libfilmCloudTransfer.so");
.
.
.
surfaceFilmModel cloudFilmTransfer;
and the film filmCloudTransfer specified in the <film> region
constant/<film>/fvModels dictionary:
.
.
.
filmCloudTransfer
{
type filmCloudTransfer;
libs ("libfilmCloudTransfer.so");
}
For an example of cloud->film->VoF transfer see the
tutorials/modules/multiRegion/film/cylinder tutorial case.
Note that parcel transfer from film to Lagrangian cloud is not yet supported,
this will be added soon.
foamToC: New run-time selection table of contents printing and interrogation utility
The new solver modules cannot provide the equivalent functionality of the -list
options available in the solver applications so foamToC has been developed as a
better, more general and flexible alternative, providing a means to print any or
all run-time selection tables in any or all libraries and search the tables for
any particular entries and print which library files the corresponding tables
are in, e.g.
foamToC -solver fluid -table fvPatchScalarField
Contents of table fvPatchScalarField, base type fvPatchField:
advective libfiniteVolume.so
calculated libfiniteVolume.so
codedFixedValue libfiniteVolume.so
codedMixed libfiniteVolume.so
compressible::alphatJayatillekeWallFunctionlibthermophysicalTransportModels.so
compressible::alphatWallFunction libthermophysicalTransportModels.so
compressible::thermalBaffle1D<eConstSolidThermoPhysics>libthermophysicalTransportModels.so
compressible::thermalBaffle1D<ePowerSolidThermoPhysics>libthermophysicalTransportModels.so
compressible::turbulentTemperatureCoupledBaffleMixedlibthermophysicalTransportModels.so
compressible::turbulentTemperatureRadCoupledMixedlibthermophysicalTransportModels.so
.
.
.
foamToC -solver fluid -search compressible::alphatWallFunction
compressible::alphatWallFunction is in tables
fvPatchField
fvPatchScalarField libthermophysicalTransportModels.so
and the very useful -allLibs option allows ALL libraries to be searched to find
in which table and which library file a particular model in in for example:
foamToC -allLibs -search phaseTurbulenceStabilisation
Loading libraries:
libtwoPhaseSurfaceTension.so
libcv2DMesh.so
libODE.so
.
.
.
phaseTurbulenceStabilisation is in tables
fvModel libmultiphaseEulerFoamFvModels.so
Application
foamToC
Description
Run-time selection table of contents printing and interrogation.
The run-time selection tables are populated by the optionally specified
solver class and any additional libraries listed in the \c -libs option or
all libraries using the \c -allLibs option. Once populated the tables can
be searched and printed by a range of options listed below. Table entries
are printed with the corresponding library they are in to aid selection
and the addition of \c libs entries to ensure availability to the solver.
Usage
\b foamToC [OPTION]
- \par -solver \<name\>
Specify the solver class
- \par -libs '(\"lib1.so\" ... \"libN.so\")'
Specify the additional libraries to load
- \par -allLibs
Load all libraries
- \par switches,
List all available debug, info and optimisation switches
- \par all,
List the contents of all the run-time selection tables
- \par tables
List the run-time selection table names (this is the default action)
- \par table \<name\>
List the contents of the specified table or the list sub-tables
- \par search \<name\>
Search for and list the tables containing the given entry
- \par scalarBCs,
List scalar field boundary conditions (fvPatchField<scalar>)
- \par vectorBCs,
List vector field boundary conditions (fvPatchField<vector>)
- \par functionObjects,
List functionObjects
- \par fvModels,
List fvModels
- \par fvConstraints,
List fvConstraints
Example usage:
- Print the list of scalar boundary conditions (fvPatchField<scalar>)
provided by the \c fluid solver without additional libraries:
\verbatim
foamToC -solver fluid -scalarBCs
\endverbatim
- Print the list of RAS momentum transport models provided by the
\c fluid solver:
\verbatim
foamToC -solver fluid -table RAScompressibleMomentumTransportModel
\endverbatim
- Print the list of functionObjects provided by the
\c multicomponentFluid solver with the libfieldFunctionObjects.so
library:
\verbatim
foamToC -solver multicomponentFluid \
-libs '("libfieldFunctionObjects.so")' -functionObjects
\endverbatim
- Print a complete list of all run-time selection tables:
\verbatim
foamToC -allLibs -tables
or
foamToC -allLibs
\endverbatim
- Print a complete list of all entries in all run-time selection tables:
\verbatim
foamToC -allLibs -all
\endverbatim
executed with foamRun for single region simulations of foamMultiRun for
multi-region simulations. Replaces driftFluxFoam and all the corresponding
tutorials have been updated and moved to
tutorials/modules/incompressibleDriftFlux.
Class
Foam::solvers::incompressibleDriftFlux
Description
Solver module for 2 incompressible fluids using the mixture approach with
the drift-flux approximation for relative motion of the phases, 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 with mixture transport modelling 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.
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
incompressibleDriftFlux.C
See also
Foam::solvers::VoFSolver
Foam::solvers::twoPhaseVoFSolver
Foam::solvers::compressibleVoF
A constraint and a model have been added, both called
zeroDimensionalFixedPressure, that together act to maintain a pressure
constraint in a zero-dimensional case. These must be used
simultaneously. The desired pressure can be specified as a time-varying
Function1.
These replace the pressureConstraintSource, which has been removed.
The new classes operate by obtaining the residual of the complete
pressure equation, and using that to calculate the mass or volume
sources that need adding to the fluid in order to maintain the
constraint. This process is far more convergent than the previous
approach, it does not require the fluid to have a certain thermodynamic
model, and it is generalisable to multiphase.
This functionality requires only minimal specification. The constraint
contains all the settings and should be specified in
system/fvConstraints as follows:
zeroDimensionalFixedPressure1
{
type zeroDimensionalFixedPressure;
// Name of the pressure field, default = p
//p p;
// Name of the density field, default = rho
//rho rho;
// Constant pressure value
pressure 1e5;
//// Time-varying pressure value
//pressure
//{
// type table;
// values
// (
// (0 1e5)
// (1 1e5)
// (1.1 1.4e5)
// (10 1.4e5)
// );
//}
}
The model is then added to constant/fvModels, and requires no settings:
zeroDimensionalFixedPressure1
{
type zeroDimensionalFixedPressure;
}
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.
executed with foamRun for single region simulations of foamMultiRun for
multi-region simulations. Replaces denseParticleFoam and all the corresponding
tutorials have been updated and moved to
tutorials/modules/incompressibleDenseParticleFluid.
Class
Foam::solvers::incompressibleDenseParticleFluid
Description
Solver module for transient flow of incompressible isothermal fluids coupled
with particle clouds including the effect of the volume fraction of
particles on the continuous phase, with optional mesh motion and change.
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, constraining or limiting
the solution.
to provide consistent and stable continuous phase velocity solution without
staggering patterns at the boundary with packed regions of dispersed phase.
If divU is valid the velocity divergence is included in the pcorr equation.
This simplifies the logic in multiphase moveMesh functions supporting
incompressible (with or without mass sources) and compressible fluids.
The cell-base momentum/pressure algorithm in the multiphaseEuler solver module
has been substantially updated to improve consistency, conservation and reduce
drag generated staggering patterns at sharp interfaces and the boundaries with
stationary phases. For most if not all cases this new algorithm can be used to
provide well resolved and reliable solutions where the faceMomentum algorithm
would have been chosen previously in order to obtain sufficiently smooth
solutions but at the expense of a noticeable loss in accuracy and resolution.
The first significant change in the momentum/pressure algorithm is in the
interpolation practice used to construct the flux predictor equation from the
cell momentum equation: rather than interpolating the H/A ratio to the faces
i.e. (H/A)_f the terms in the momentum equation are interpolated separately so
that H_f/A_f is used. The same approach is used for the drag i.e. (D_f/A_f) and
virtual mass contributions. The advantage of this change is that the phase
forces are now consistent in both the momentum and flux equations, i.e. sum to
zero for each pair of phases.
The second significant change is in the handling of ddtCorr which converts the
old-time time-derivative contributions in H from velocity to flux which is now
consistent due to the change to H/A interpolation and also generalised to use
the fvc::ddtCorr function which has been updated for multiphase. Additionally
ddtCorr may optionally be applied to the time-derivative in the virtual mass
term in a consistent manner so that the contributions to the flux equation sum
to zero for each pair of phases.
The third significant change is the addition of an optional drag correction term
to the momentum corrector to reduce the staggering patters generated in the
velocity field due to sudden changes in drag force between phase, e.g. at sharp
interfaces between phases or at the boundaries with stationary phases. This is
particularly beneficial for fluidised bed simulations. However this correction
is not and cannot be phase consistent, i.e. the correction does not sum to zero
for pairs of phases it is applied to so a small drag error is introduced, but
tests so far have shown that the error is small and outweighed by the benefit in
the reduction in numerical artefacts in the solution.
The final significant change is in the handling of residualAlpha for drag and
virtual mass to provide stable and physical phase velocities in the limit of the
phase-fraction -> 0. The new approach is phase asymmetric such that the
residual drag is applied only to the phase with a phase-fraction less than
residualAlpha and not to the carrier phase. This change ensures that the flow
of a pure phase is unaffected by the residualAlpha and residual drag of the
other phases that are stabilised in pure phase region.
There are now four options in the PIMPLE section of the fvSolutions dictionary
relating to the multiphase momentum/pressure algorithm:
PIMPLE
{
faceMomentum no;
VmDdtCorrection yes;
dragCorrection yes;
partialElimination no;
}
faceMomentum:
Switches between the cell and face momentum equation algorithms.
Provides much smoother and reliable solutions for even the most challenging
multiphase cases at the expense of a noticeable loss in accuracy and resolution.
Defaults to 'no'.
VmDdtCorrection:
Includes the ddtCorr correction term to the time-derivative part of the
virtual-mass term in the flux equation which ensures consistency between the
phase virtual mass force on the faces but generates solutions which are
slightly less smooth and more likely to contain numerical artefacts.
Defaults to 'no'.
Testing so far has shown that the loss in smoothness is small and there is
some noticeable improvement is some cases so in the future the default may
be changed to 'yes'.
dragCorrection:
Includes the momentum corrector drag correction term to reduce the
staggering patters generated in the velocity field due to sudden changes in
drag force at the expense of a small error in drag consistency.
Defaults to 'no'
partialElimination:
Switches the partial-elimination momentum corrector which inverts the drag
matrix for both the momentum equations and/or flux equations to provide a
drag implicit correction to the phase velocity and flux fields. The
algorithm is the same as previously but updated for the new consistent drag
interpolation.
All the tutorials/modules/multiphaseEuler tutorial cases have been updated and
tested with the above developments and the four options set appropriately for
each.
