across all the phases in an Eulerian multi-phase simulation.
Intended to be used with copiedFixedValue to ensure that phase wall
temperature are consistent:
- Set 'fixedMultiPhaseHeatFlux' boundary for one of the phases
- Use 'copiedFixedValue' for all the other phases.
Based on code provided by Juho Peltola
Provides run-time selection of buoyancy sources for compressible solvers
Replaces the built-in buoyancy sources in XiFoam, reactingFoam and
rhoReactingFoam.
e.g. in constant/fvOptions specify
momentumSource
{
type buoyancyForce;
buoyancyForceCoeffs
{
fieldNames (U);
}
}
and optionally specify the buoyancy energy source in the enthalpy
equation:
energySource
{
type buoyancyEnergy;
buoyancyEnergyCoeffs
{
fieldNames (h);
}
}
or internal energy equation
energySource
{
type buoyancyEnergy;
buoyancyEnergyCoeffs
{
fieldNames (e);
}
}
New lift model supporting near-wall damping using the new
wallDampingModels.
e.g.
lift
(
(air in water)
{
type wallDamped;
lift
{
type constantCoefficient;
Cl 0.5;
}
wallDamping
{
type linear;
Cd 0.5;
}
}
);
in which a linear near-wall damping function min(y/(Cd*d), 1) is applied to the constant
coefficient lift model. Additional wall-damping functions will be added.
to allow iteration over the energy equations to improve stability for phase-change.
Additionally if nEnergyCorrectors is set to 0 the energy equations are
not solved which may be beneficial during the startup of some cases.
Now solvers return solver performance information for all components
with backward compatibility provided by the "max" function which created
the scalar solverPerformance from the maximum component residuals from
the SolverPerformance<Type>.
The residuals functionObject has been upgraded to support
SolverPerformance<Type> so that now the initial residuals for all
(valid) components are tabulated, e.g. for the cavity tutorial case the
residuals for p, Ux and Uy are listed vs time.
Currently the residualControl option of pimpleControl and simpleControl
is supported in backward compatibility mode (only the maximum component
residual is considered) but in the future this will be upgraded to
support convergence control for the components individually.
This development started from patches provided by Bruno Santos, See
http://www.openfoam.org/mantisbt/view.php?id=1824
to allow the turbulent energy transport properties to be updated for
every energy solution if required.
Added correctEnergyTransport() call to reactingTwoPhaseEulerFoam
so that the specification of the name and dimensions are optional in property dictionaries.
Update tutorials so that the name of the dimensionedScalar property is
no longer duplicated but optional dimensions are still provided and are
checked on read.
The interfacial temperature is assumed equal to the saturation
temperature. Only a single species is considered volatile and the other
species to not affect the mass-transfer.
Added calls to setFluxRequired for p in all incompressible solvers which
avoids the need to add fluxRequired entries in fvSchemes dictionary.
Will add calls to setFluxRequired to the rest of the solvers.
Currently this is implemented only for the Antoine equation, for the
other more complex models an iterative inversion from pressure to
temperature is required.
Select using the optional
consistent true;
setting in the PIMPLE dictionary of fvSolution.
This option is generally only beneficial for cases run in PIMPLE-mode
with a large maximum Courant number.
Select LTS via the ddtScheme:
ddtSchemes
{
default localEuler rDeltaT;
}
The LTS algorithm is currently controlled with the standard settings in
controlDict, e.g.:
maxCo 0.5;
maxDeltaT 2e-8;
with the addition of the optional rDeltaT smoothing coefficient:
rDeltaTSmoothingCoeff 0.02;
which defaults to 0.02.
ddtSchemes
{
default localEuler rDeltaT;
}
LTS is selected by the ddt scheme e.g. in the
tutorials/multiphase/interFoam/ras/DTCHull case:
ddtSchemes
{
default localEuler rDeltaT;
}
LTSInterFoam is no longer needed now that interFoam includes LTS
support.
to support laminar simulations in the new framework.
Unfortunately this allows LES models to be instantiated although they
are not compatible with steady-state simulations.
Select LTS via the ddtScheme:
ddtSchemes
{
default localEuler rDeltaT;
}
The LTS algorithm is controlled with the standard settings in
controlDict, e.g.:
maxCo 0.5;
maxDeltaT 2e-8;
with the addition of the optional rDeltaT smoothing coefficient:
rDeltaTSmoothingCoeff 0.02;
which defaults to 0.02.
For cases with reasonably uniform meshes like the forwardStep tutorial
LTS does not provide much benefit but for cases with large variation in
cell-size like the biconic25-55Run35 tutorial LTS provides significant
speed-up to convergence particularly if started from uniform conditions.
Reverted changes proposed in
http://openfoam.org/mantisbt/view.php?id=1548 as it adversely affects
fixed-value BCs and is formulated to fix an issue with an unphysical
case. Further analysis of the handling of fixed pressure outlet
conditions as the Mach number approaches 1 is required.
Multi-species, mass-transfer and reaction support and multi-phase
structure provided by William Bainbridge.
Integration of the latest p-U and face-p_U algorithms with William's
multi-phase structure is not quite complete due to design
incompatibilities which needs further development. However the
integration of the functionality is complete.
The results of the tutorials are not exactly the same for the
twoPhaseEulerFoam and reactingTwoPhaseEulerFoam solvers but are very
similar. Further analysis in needed to ensure these differences are
physical or to resolve them; in the meantime the twoPhaseEulerFoam
solver will be maintained.
Model which applies an analytical solution for heat transfer from the
surface of a sphere to the fluid within the sphere.
Provided by William Bainbridge
fvOptions does not have the appropriate structure to support MRF as it
is based on option selection by user-specified fields whereas MRF MUST
be applied to all velocity fields in the particular solver. A
consequence of the particular design choices in fvOptions made it
difficult to support MRF for multiphase and it is easier to support
frame-related and field related options separately.
Currently the MRF functionality provided supports only rotations but
the structure will be generalized to support other frame motions
including linear acceleration, SRF rotation and 6DoF which will be
run-time selectable.
SIMPLEC (SIMPLE-consistent) is selected by setting "consistent" option true/yes:
SIMPLE
{
nNonOrthogonalCorrectors 0;
consistent yes;
}
which relaxes the pressure in a "consistent" manner and additional
relaxation of the pressure is not generally necessary. In addition
convergence of the p-U system is better and reliable with less
aggressive relaxation of the momentum equation, e.g. for the motorbike
tutorial:
relaxationFactors
{
equations
{
U 0.9;
k 0.7;
omega 0.7;
}
}
The cost per iteration is marginally higher but the convergence rate is
better so the number of iterations can be reduced.
The SIMPLEC algorithm also provides benefit for cases with large
body-forces, e.g. SRF, see tutorials/incompressible/SRFSimpleFoam/mixer
and feature request http://www.openfoam.org/mantisbt/view.php?id=1714
Rather than forcing the dispersed-phase velocity -> the continuous-phase
velocity as the phase-fraction -> 0 the velocity is now calculated from
a balance of pressure, buoyancy and drag forces. The advantage is now
liquid or particles are not carried out of bubble-column of
fluidised-beds by the fictitious drag caused by forcing the
phase-velocities becoming equal in the limit.
nLimiterIter: Number of iterations during limiter construction
3 (default) is sufficient for 3D simulations with a Courant number 0.5 or so
For larger Courant numbers larger values may be needed but this is
only relevant for IMULES and CMULES
smoothLimiter: Coefficient to smooth the limiter to avoid "diamond"
staggering patters seen in regions of low particle phase-fraction in
fluidised-bed simulations.
The default is 0 as it is not needed for all simulations.
A value of 0.1 is appropriate for fluidised-bed simulations.
The useful range is 0 -> 0.5.
Values larger than 0.5 may cause excessive smearing of the solution.
This formulation provides C-grid like pressure-flux staggering on an
unstructured mesh which is hugely beneficial for Euler-Euler multiphase
equations as it allows for all forces to be treated in a consistent
manner on the cell-faces which provides better balance, stability and
accuracy. However, to achieve face-force consistency the momentum
transport terms must be interpolated to the faces reducing accuracy of
this part of the system but this is offset by the increase in accuracy
of the force-balance.
Currently it is not clear if this face-based momentum equation
formulation is preferable for all Euler-Euler simulations so I have
included it on a switch to allow evaluation and comparison with the
previous cell-based formulation. To try the new algorithm simply switch
it on, e.g.:
PIMPLE
{
nOuterCorrectors 3;
nCorrectors 1;
nNonOrthogonalCorrectors 0;
faceMomentum yes;
}
It is proving particularly good for bubbly flows, eliminating the
staggering patterns often seen in the air velocity field with the
previous algorithm, removing other spurious numerical artifacts in the
velocity fields and improving stability and allowing larger time-steps
For particle-gas flows the advantage is noticeable but not nearly as
pronounced as in the bubbly flow cases.
Please test the new algorithm on your cases and provide feedback.
Henry G. Weller
CFD Direct
