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.
Horizontal mixers have been renamed to mixerVesselHorizontal2D. The
incompressible mixerVessel2D has been reinstated to provide a comparison
with the corresponding MRF case. All rotational speeds have been
standardised at 60 rpm, except for the compressible case in which the
higher speed is justified in order to demonstrate the simulation of
compressibility effects.
The codedFunctionObjectTemplate is based on regionFunctionObject requiring
fvMesh.H and most manipulate volFields so it makes sense for volFields.H to be
included by default.
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.
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.
Demonstration case for three region coupling with film consisting of an
aluminium panel with surface film running down forming rivulets in a box of air
which moved due to buoyancy with 6-way thermal and velocity coupling between the
panel<->film<->air<->panel. The case runs serial and parallel with arbitrary
decomposition.
Currently extrudeToRegionMesh does not directly support three region coupling so
foamDictionary is used to edit the of the boundary files of box and film regions
to add box<->film coupling.
genericPatches is linked into mesh generation and manipulation utilities but not
solvers so that the solvers now check for the availability of the specified
patch types. Bugs in the tutorials exposed by this check have been corrected.
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.
This change applies to diameter models within the multiphaseEuler
module, heat transfer fvModels, and the LopesdaCosta porosity and
turbulence models.
User input changes have been made backwards-compatible, so existing
AoV/a/Sigma/... entries and fields should continue to work.
Two pitzDaily variants have been added; pitzDailySteadyMappedToPart, and
pitzDailySteadyMappedToRefined. These demonstrate usage of workflows
which involve mapping between cases with mapFieldsPar.
The pitzDailySteadyMappedToPart case demonstrates mapping onto a small
section of the mesh; in this case in the vicinity of the the corner of
the backstep. This mesh is not consistent with the source data, so
fields are required in the zero directory and cutting patches are used
to specify the properties at the inlets.
The pitzDailySteadyMappedToRefined case demonstrates mapping onto a
geometrically similar case with a different mesh density. This mesh is
consistent with the source, so no fields are needed and no cutting
patches are used. This case does, however, perturb the geometry of the
block mesh a bit, so that some of the refined case is not overlapping
the original case. This provides a test of the stabilisation
procedures within the mesh-to-mesh mapping functions.
Cell-to-cell interpolation has been moved to a hierarchy separate from
meshToMesh, called cellsToCells. The meshToMesh class is now a
combination of a cellsToCells object and multiple patchToPatch objects.
This means that when only cell-to-cell interpolation is needed a basic
cellsToCells object can be selected.
Cell-to-cell and vol-field-to-vol-field interpolation now has two well
defined sets of functions, with a clear distinction in how weights that
do not sum to unity are handled. Non-unity weights are either
normalised, or a left-over field is provided with which to complete the
weighted sum.
The left-over approach is now consistently applied in mapFieldsPar,
across both the internal and patch fields, if mapping onto an existing
field in the target case. Warning are now generated for invalid
combinations of settings, such as mapping between inconsistent meshes
without a pre-existing target field.
All mapping functions now take fields as const references and return tmp
fields. This avoids the pattern in which non-const fields are provided
which relate to the source, and at some point in the function transfer
to the target. This pattern is difficult to reason about and does not
provide any actual computational advantage, as the fields invariably get
re-allocated as part of the process anyway.
MeshToMesh no longer stores the cutting patches. The set of cutting
patches is not needed anywhere except at the point of mapping a field,
so it is now supplied to the mapping functions as an argument.
The meshToMesh topology changer no longer supports cutting patch
information. This did not previously work. Cutting patches either get
generated as calculated, or they require a pre-existing field to specify
their boundary condition. Neither of these options is suitable for a
run-time mesh change.
More code has been shared with patchToPatch, reducing duplication.
Solvers ensure fluxes are maintained and updated correctly after topology change
and it no longer the responsibility of fvMeshTopoChangersRefiner to attempt
this.
The '-region' option has been leveraged to significantly simplify the
meshing and decomposition in the movingCone cases. These cases have also
been corrected to restore the variation in decomposition between the
different meshes, which is important for thoroughly testing the patch
field mapping. The shockFluid case has also had its duration extended a
little in order to span the final mesh mapping time.
The method to update phi in PDRFoamAutoRefine has been superseded by rhoUf in
all other compressible solvers and PDRFoam needs to be updated, requiring
funding. PDRFoamAutoRefine is no longer maintained.
The keyword 'select' is now used to specify the cell, face or point set
selection method consistently across all classes requiring this functionality.
'select' replaces the inconsistently named 'regionType' and 'selectionMode'
keywords used previously but backwards-compatibility is provided for user
convenience. All configuration files and tutorials have been updated.
Examples of 'select' from the tutorial cases:
functionObjects:
cellZoneAverage
{
type volFieldValue;
libs ("libfieldFunctionObjects.so");
writeControl writeTime;
writeInterval 1;
fields (p);
select cellZone;
cellZone injection;
operation volAverage;
writeFields false;
}
#includeFunc populationBalanceSizeDistribution
(
name=numberDensity,
populationBalance=aggregates,
select=cellZone,
cellZone=outlet,
functionType=numberDensity,
coordinateType=projectedAreaDiameter,
allCoordinates=yes,
normalise=yes,
logTransform=yes
)
fvModel:
cylinderHeat
{
type heatSource;
select all;
q 5e7;
}
fvConstraint:
momentumForce
{
type meanVelocityForce;
select all;
Ubar (0.1335 0 0);
}
This is a more intuitive keyword than "funcName" or "entryName". A
function object's name and corresponding output directory can now be
renamed as follows:
#includeFunc patchAverage
(
name=cylinderT, // <-- was funcName=... or entryName=...
region=fluid,
patch=fluid_to_solid,
field=T
)
Some packaged functions previously relied on a "name" argument that
related to an aspect of the function; e.g., the name of the faceZone
used by the faceZoneFlowRate function. These have been disambiguated.
This has also made them consistent with the preferred input syntax of
the underlying function objects.
Examples of the changed #includeFunc entries are shown below:
#includeFunc faceZoneAverage
(
faceZone=f0, // <-- was name=f0
U
)
#includeFunc faceZoneFlowRate
(
faceZone=f0 // <-- was name=f0
)
#includeFunc populationBalanceSizeDistribution
(
populationBalance=bubbles,
regionType=cellZone,
cellZone=injection, // <-- was name=injection
functionType=volumeDensity,
coordinateType=diameter,
normalise=yes
)
#includeFunc triSurfaceAverage
(
triSurface=mid.obj, // <-- was name=mid.obj
p
)
#includeFunc triSurfaceVolumetricFlowRate
(
triSurface=mid.obj // <-- was name=mid.obj
)
#includeFunc uniform
(
fieldType=volScalarField,
fieldName=alpha, // <-- was name=alpha
dimensions=[0 0 0 0 0 0 0],
value=0.2
)
