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.
The mixture compressibility/density is now included in CorrectPhi for
compressible mixtures, consistent with the compressibility handling in the
pressure equation. This improves consistency, robustness and convergence of the
pcorr equation.
so that the residualAlpha applied to stabilised the dispersed phase does not
affect the continuous phase in the limit of it becoming pure with or without
partial-elimination.
Flux correction is now applied if either the topology changed or the mesh is
moving and correctPhi is true. This strategy allows moving mesh cases without
topology change to be run without any change to the fluxes which is appropriate
for solid-body motion of the entire domain or a rotating sub-domain with NCC.
Class
Foam::solvers::functions
Description
Solver module to execute the \c functionObjects for a specified solver
The solver specified by either the \c subSolver or if not present the \c
solver entry in the \c controlDict is instantiated to provide the physical
fields needed by the \c functionObjects. The \c functionObjects are then
instantiated from the specifications are read from the \c functions entry in
the \c controlDict and executed in a time-loop also controlled by entries in
\c controlDict and the \c maxDeltaT() returned by the sub-solver.
The fields and other objects registered by the sub-solver are set to
NO_WRITE as they are not changed by the execution of the functionObjects and
should not be written out each write-time. Fields and other objects created
and changed by the execution of the functionObjects are written out.
When restarting from a time directory which does contain the \c subSolver
fields the optional \c controlDict entry \c subSolverTime may be provided to
specify which time the \c subSolver should be instantiated for, after which
time is reset to \c startTime for the restart.
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.
These two new fvModels operate between a film and a VoF region to transfer film
to the corresponding VoF phase when the film is thick enough to be resolved by
the VoF solver or from the VoF phase to the film when the near-wall resolution
is too low and it is better to treat it as a wall film.
This functionality is equivalent to the VoFPatchTransfer fvModel developed for
the old film implementation but coded in a much more general manner with
implicit treatment of the mass loss from the film or VoF region for better
numerical stability and robustness.
The simple tutorials/modules/CHT/VoFToFilm case is provided to demonstrate a
film being deposited on a surface as the plate is withdrawn from a liquid. It
is an updated version of the tutorials/modules/compressibleVoF/plateFilm case.
Class
Foam::filmSurfaceVelocityFvPatchVectorField
Description
Film surface velocity boundary condition
Evaluates the surface velocity from the shear imposed by the neighbouring
fluid velocity using either a simple drag model based on the difference
between the fluid and film velocities multiplied by the coefficient \c Cs or
if \c Cs is not specified or set to 0 the fluid viscous shear stress.
The simple model might be used in preference to the fluid viscous shear
stress model in order to provide some means to include the drag enhancing
effect of surface ripples, rivulets etc. in the film surface.
Usage
\table
Property | Description | Required | Default value
Cs | Fluid-film drag coefficient | no | 0
\endtable
Example of the boundary condition specification using the simple drag model:
\verbatim
<patchName>
{
type filmSurfaceVelocity;
Cs 0.005;
value $internalField;
}
\endverbatim
Example of the boundary condition specification using the fluid stress:
\verbatim
<patchName>
{
type filmSurfaceVelocity;
value $internalField;
}
\endverbatim
See also
Foam::mixedFvPatchField
SourceFiles
filmSurfaceVelocityFvPatchVectorField.C
e.g. for the rivuletBox case the output for a time-step now looks like:
film Courant Number mean: 0.0003701330848 max: 0.1862204919
panel Diffusion Number mean: 0.007352456305 max: 0.1276468109
box Courant Number mean: 0.006324172752 max: 0.09030825997
deltaT = 0.001550908752
Time = 0.08294s
film diagonal: Solving for alpha, Initial residual = 0, Final residual = 0, No Iterations 0
film diagonal: Solving for alpha, Initial residual = 0, Final residual = 0, No Iterations 0
box diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
film DILUPBiCGStab: Solving for Ux, Initial residual = 0.009869417958, Final residual = 2.132619614e-11, No Iterations 2
film DILUPBiCGStab: Solving for Uy, Initial residual = 0.0002799662756, Final residual = 6.101011285e-12, No Iterations 1
film DILUPBiCGStab: Solving for Uz, Initial residual = 1, Final residual = 1.854120599e-12, No Iterations 2
box DILUPBiCGStab: Solving for Ux, Initial residual = 0.004071057403, Final residual = 4.79249226e-07, No Iterations 1
box DILUPBiCGStab: Solving for Uy, Initial residual = 0.006370817152, Final residual = 9.606673696e-07, No Iterations 1
box DILUPBiCGStab: Solving for Uz, Initial residual = 0.0158299327, Final residual = 2.104129791e-06, No Iterations 1
film DILUPBiCGStab: Solving for e, Initial residual = 0.0002888908396, Final residual = 2.301587523e-11, No Iterations 1
panel GAMG: Solving for e, Initial residual = 0.00878508958, Final residual = 7.807579738e-12, No Iterations 1
box DILUPBiCGStab: Solving for h, Initial residual = 0.004403989559, Final residual = 1.334113552e-06, No Iterations 1
film DILUPBiCGStab: Solving for alpha, Initial residual = 0.0002760406755, Final residual = 2.267583256e-14, No Iterations 1
film time step continuity errors : sum local = 9.01334987e-12, global = 2.296671859e-13, cumulative = 1.907846466e-08
box GAMG: Solving for p_rgh, Initial residual = 0.002842335602, Final residual = 1.036572819e-05, No Iterations 4
box diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
box time step continuity errors : sum local = 4.538744531e-07, global = 1.922637799e-08, cumulative = -6.612579497e-09
box GAMG: Solving for p_rgh, Initial residual = 1.283128787e-05, Final residual = 7.063185653e-07, No Iterations 2
box diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
box time step continuity errors : sum local = 3.069629869e-08, global = 3.780547824e-10, cumulative = -6.234524715e-09
ExecutionTime = 19.382601 s ClockTime = 20 s
film Courant Number mean: 0.0003684434169 max: 0.1840342756
panel Diffusion Number mean: 0.007352456305 max: 0.1276468109
box Courant Number mean: 0.006292704463 max: 0.09016861809
deltaT = 0.001550908752
Time = 0.0844909s
where each line printed by each region solver is prefixed by the region name.
Global messages for the time-step and time are just prefixed with spaces to
align them with the region output.
Class
Foam::filmSurfaceVelocityFvPatchVectorField
Description
Film surface velocity boundary condition
Evaluates the surface velocity from the shear imposed by the neighbouring
fluid velocity using a simple drag model based on the difference between the
fluid and film velocities multiplied by the coefficient \c Cs. This simple
model is used in preference to the standard viscous shear stress model in
order to provide some means to include the drag enhancing effect
of surface ripples, rivulets etc. in the film surface.
Usage
\table
Property | Description | Required | Default value
Cs | Fluid-film drag coefficient | yes |
\endtable
Example of the boundary condition specification:
\verbatim
<patchName>
{
type filmSurfaceVelocity;
Cs 0.005;
}
\endverbatim
mappedFilmPressureFvPatchScalarField is derived from the new mappedFvPatchField
base-class for mapped patch fields including mappedValueFvPatchField.
Class
Foam::mappedFilmPressureFvPatchScalarField
Description
Film pressure boundary condition which maps the neighbouring fluid patch
pressure to both the surface patch and internal film pressure field.
A new wallBoiling heat transfer model has been added for use with the
thermalPhaseChangeMultiphaseSystem. This model operates similarly to the
alphatWallBoilingWallFunction. The difference is that the boiling generated by
the wallBoiling heat transfer model occurs on the surface of a third stationary
phase, within the volume of the simulation, rather than on a wall patch. This
can be used to model boiling within a packed bed or similar.
The wallBoiling heat transfer model and the alphatWallBoilingWallFunction share
underlying sub-models, so their specification is very similar. For example, in
constant/phaseProperties:
heatTransfer
{
...
bed_dispersedIn_liquid_inThe_liquid
{
type wallBoiling;
liquidPhase liquid;
vapourPhase gas;
heatTransferModel
{
type Gunn;
}
partitioningModel
{
type Lavieville; // phaseFraction, linear, cosine
alphaCrit 0.2;
}
nucleationSiteModel
{
type LemmertChawla; // KocamustafaogullariIshii
}
departureDiameterModel
{
type TolubinskiKostanchuk; // KocamustafaogullariIshii
}
departureFrequencyModel
{
type KocamustafaogullariIshii; // Cole
Cf 1.18;
}
}
bed_dispersedIn_liquid_inThe_bed
{
type spherical;
}
...
}
Based on a patch contributed by Juho Peltola, VTT.
Class
Foam::solvers::film
Description
Solver module for flow of compressible liquid films
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,
radiation, surface film etc. and constraining or limiting the solution.
solvers::film is derived from solvers::isothermalFilm adding an energy equation
and temperature update with support for heat transfer to the wall using the
standard ThermophysicalTransportModels library utilising the filmWall patch type
or mappedFilmWall for CHT heat transfer to the adjacent solid region. A huge
advantage of this consistency with the rest of OpenFOAM is that the standard
thermal coupled boundary conditions can be used without modification, e.g.
temperatureCoupled.
Two variants of the rivuletPanel tutorial case are provided,
tutorials/modules/film/rivuletPanel demonstrates heat transfer to a fixed
temperature wall and tutorials/modules/CHT/rivuletPanel demonstrates conjugate
heat transfer to a thin aluminium panel simulated in a region using the
solvers::solid solver executed with solvers::film using foamMultiRun.
More functionality will be added through the power of fvModels.
Class
Foam::solvers::isothermalFilm
Description
Solver module for flow of compressible isothermal liquid films
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.
The implementation of this new film solver is in fully conservative form,
solving for the film volume-fraction rather film thickness which ensures
conservation on curved and irregular surfaces and even around corners.
Also the formulation is consistent with standard FV solvers in other fundamental
respects using boundary conditions rather than volume forces to apply surface
stresses and transfers. This hugely advantageous approach, which allows the
reuse of many of the standard OpenFOAM libraries, in particular standard
compressibleMomentumTransportModels for the wall and internal film stresses, is
achieved using the special patch types filmWall and filmSurface to handle the
difference between the film thickness and the film cell layer height.
The specification of physical properties, boundary conditions, optional models
etc. etc. is handled in the same manner as all the other solver modules, making
much easier to use and to maintain the code.
Currently only coupling to the wall is supported with laminar transport, surface
tension, a new and more accurate contact angle algorithm and gravity which is
sufficient to demonstrate rivulet flow for example as in the tutorial case
provided: tutorials/modules/isothermalFilm/rivuletPanel
Support for coupling to an adjacent fluid region, Lagrangian impingement and
ejection, transfer to and from a VoF phase etc. will be added in the future via
the standard fvModels interface.
