Rather than specifying the controls per field it is simpler to use a single set
of controls for all the fields in the list and use separate instances of the
fieldAverage functionObject for different control sets:
Example of function object specification setting all the optional parameters:
fieldAverage1
{
type fieldAverage;
libs ("libfieldFunctionObjects.so");
writeControl writeTime;
restartOnRestart false;
restartOnOutput false;
periodicRestart false;
restartPeriod 0.002;
base time;
window 10.0;
windowName w1;
mean yes;
prime2Mean yes;
fields (U p);
}
This allows for a simple specification with the optional prime2Mean entry using
#includeFunc fieldAverage(U, p, prime2Mean = yes)
or if the prime2Mean is not needed just
#includeFunc fieldAverage(U, p)
The mean, prime2Mean and base now have default values:
{
mean on; // (default = on)
prime2Mean on; // (default = off)
base time; // time or iteration (default = time)
window 200; // optional averaging window
windowName w1; // optional window name (default = "")
}
so for the majority of cases for which these defaults are appropriate the
fieldAverage functionObject can now be specified in the functions entry in
controlDict thus:
functions
{
fieldAverage1
{
#includeEtc "caseDicts/postProcessing/fields/fieldAverage.cfg"
fields
(
U.air
U.water
alpha.air
p
);
}
}
also utilising the new fieldAverage.cfg file.
For cases in which these defaults are not appropriate, e.g. the prime2Mean is
also required the optional entries can be specified within sub-dictionaries for
each field, e.g.
fieldAverage1
{
#includeEtc "caseDicts/postProcessing/fields/fieldAverage.cfg"
fields
(
U
{
prime2Mean yes;
}
p
{
prime2Mean yes;
}
);
}
The hRefConst and eRefConst thermos that were local to
reacting*EulerFoam have been removed and the reference state that they
used has been incorporated into the standard hConst and eConst thermos.
The hConst thermo model now evaluates the enthalpy like so:
Ha = Hf + Hs
= Hf + Cp*(T - Tref) + Hsref (+ equation of state terms)
Where Ha is absolute enthalpy, Hs is sensible enthalpy, Cp is specific
heat at constant pressure, T is temperature, Tref is a reference
temperature and Hsref is a reference sensible enthalpy. Hf, Cp, Tref and
Hsref are user inputs. Of these, Tref and Hsref are new. An example
specification is as follows:
thermodynamics
{
Hf -1.34229e+07;
Cp 2078.4;
Tref 372.76;
Hsref 128652;
}
The ref quantities allows the user to specify a state around which to
linearise the relationship between temperature and enthalpy. This is
useful if the temperature range of the simulation is small enough to
consider the relationship linear, but linearity does not hold all the
way to standard conditions.
To maintain backwards compatibility, Tref defaults to standard
temperature, and Hsref defaults to zero, so a case using hConst thermo
requires no modification as a result of this change.
The only change to the default operation is that to calculate sensible
enthalpy Cp is multiplied by the difference between the current
temperature and the standard temperature, whether as previously Cp was
multiplied by the current temperature only. This means that at standard
conditions sensible enthalpy is now zero, and absolute enthalpy equals
the formation enthalpy. This is more consistent with the definitions of
the various enthalpies, and with other thermo models such as janaf. This
change should only affect reacting cases that use constant thermo
models.
This case is an updated version of
tutorials/multiphase/multiphaseEulerFoam/damBreak4phase using the latest models
available in reactingMultiphaseEulerFoam for interface capturing.
In multiphase systems it is only necessary to solve for all but one of the
moving phases. The new referencePhase option allows the user to specify which
of the moving phases should not be solved, e.g. in constant/phaseProperties of the
tutorials/multiphase/reactingMultiphaseEulerFoam/RAS/fluidisedBed tutorial case with
phases (particles air);
referencePhase air;
the particles phase is solved for and the air phase fraction and fluxes obtained
from the particles phase which provides equivalent behaviour to
reactingTwoPhaseEulerFoam and is more efficient than solving for both phases.
The thermal phase system now operates with saturation models specified
per phase-pair, and can therefore represent multiple transfer processes
across different interfaces. There is no longer a "phaseChange" switch;
instead the selection of a saturation model for a given interface
enables phase change across that interface. This includes both
interfacial phase change and nucleate wall boiling.
Both interfacial phase change and wall boiling models now include
support for there being a single specified volatile component which
undergoes phase change.
A correction has been made to the phase change energy transfer when only
interfacial phase change is enabled.
The thermal phase change tutorials have all been updated to reflect
these changes in the user interface.
Patch contributed by Juho Peltola, VTT.
The kOmegaSSTSata model can now be used in multiphase cases, provided
that there is a single, well defined continuous phase. As previously,
the continuous phase is the phase for which the model is selected (i.e.,
in the constant/turbulenceProperties.<continuous-phase-name>
dictionary).
By default, now, all other moving phases are considered to be dispersed
bubble phases, and the effect of all of them is summed to calculate the
overall bubble induced turbulence.
This behaviour can be overridden by means of a "dispersedPhases" entry,
which takes a list of the phases to be considered dispersed by the
model.
Patch contributed by Timo Niemi, VTT.
Function1 has been generalised in order to provide functionality
previously provided by some near-duplicate pieces of code.
The interpolationTable and tableReader classes have been removed and
their usage cases replaced by Function1. The interfaces to Function1,
Table and TableFile has been improved for the purpose of using it
internally; i.e., without user input.
Some boundary conditions, fvOptions and function objects which
previously used interpolationTable or other low-level interpolation
classes directly have been changed to use Function1 instead. These
changes may not be backwards compatible. See header documentation for
details.
In addition, the timeVaryingUniformFixedValue boundary condition has
been removed as its functionality is duplicated entirely by
uniformFixedValuePointPatchField.
Mass transfer rates now have a more comprehensive naming convention.
"dmdt" means a bulk/mixture transfer, whilst "dmidt" is for a
specie-specific transfer. "dmdt" implies a transfer into a phase, whilst
"dmdtf" means a transfer across an interface. Tables or lists of
transfers are denoted by pluralising the name with the suffix "s"; e.g.,
"dmdtfs". All registered mass transfer rate fields have names which
include the name of the sub-model or phase system which generated them.
The phaseTransfer models have been changed so that the mixture and the
specie-specific mass transfers are independent. This simplifies the
naming convention required for registering the resulting mass transfers
and reduces the amount of logic necessary in the phase system.
The inheritance pattern of the alphat wall functions has been altered so
that the code and parameters relating to phase change are reused, and so
that the base (the Jayatilleke wall function) more closely resembles the
library implementation. This should make it easier to remove it when the
library function is generalised enough to use it directly.
The phaseSystem::zero*Field construction functions have been removed as
their behaviour regarding registration was not clear, and in most
instances of their usage the GeometriField<...>::New methods are
similarly convenient.
Description
Reciprocal polynomial equation of state for liquids and solids
\f[
1/\rho = C_0 + C_1 T + C_2 T^2 - C_3 p - C_4 p T
\f]
This polynomial for the reciprocal of the density provides a much better fit
than the equivalent polynomial for the density and has the advantage that it
support coefficient mixing to support liquid and solid mixtures in an
efficient manner.
Usage
\table
Property | Description
C | Density polynomial coefficients
\endtable
Example of the specification of the equation of state for pure water:
\verbatim
equationOfState
{
C (0.001278 -2.1055e-06 3.9689e-09 4.3772e-13 -2.0225e-16);
}
\endverbatim
Note: This fit is based on the small amount of data which is freely
available for the range 20-65degC and 1-100bar.
This equation of state is a much better fit for water and other liquids than
perfectFluid and in general polynomials for the reciprocal of the density
converge much faster than polynomials of the density. Currently rPolynomial is
quadratic in the temperature and linear in the pressure which is sufficient for
modest ranges of pressure typically encountered in CFD but could be extended to
higher order in pressure and/temperature if necessary. The other huge advantage
in formulating the equation of state in terms of the reciprocal of the density
is that coefficient mixing is simple.
Given these advantages over the perfectFluid equation of state the libraries and
tutorial cases have all been updated to us rPolynomial rather than perfectFluid
for liquids and water in particular.
This change adds representation of the shape of a dispersed phase. A
layer has been added to model the relationship between the
characteristic volume of a sizeGroup and its physical diameter.
Previously this relationship was represented by a constant form factor.
Currently, two shape models are available:
- spherical
- fractal (for modelling fractal agglomerates)
The latter introduces the average surface area to volume ratio, kappa,
of the entities in a size group as a secondary field-dependent internal
variable to the population balance equation, which makes the population
balance approach "quasi-"bivariate. From kappa and a constant mass
fractal dimension, a collisional diameter can be derived which affects
the coagulation rates computed by the following models:
- ballisticCollisions
- brownianCollisions
- DahnekeInterpolation
- turbulentShear
The fractal shape modelling also takes into account the effect of sintering
of primary particles on the surface area of the aggregate.
Further additions/changes:
- Time scale filtering for handling large drag and heat transfer
coefficients occurring for particles in the nanometre range
- Aerosol drag model based on Stokes drag with a Knudsen number based
correction (Cunningham correction)
- Reaction driven nucleation
- A complete redesign of the sizeDistribution functionObject
The functionality is demonstrated by a tutorial case simulating the
vapour phase synthesis of titania by titanium tetrachloride oxidation.
Patch contributed by Institute of Fluid Dynamics, Helmholtz-Zentrum Dresden -
Rossendorf (HZDR) and VTT Technical Research Centre of Finland Ltd.
All reactingEulerFoam wall boiling tutorials have been replaced with
cases that are more representative of real applications.
The wall boiling tutorials for reactingTwoPhaseEulerFoam are:
RAS/wallBoiling:
Axi-symmetric wall boiling case with constant bubble diameter
RAS/wallBoilingPolyDisperse:
As wallBoiling, but with a homogenous class method population
balance for modelling the bubble diameters
RAS/wallBoilingIATE:
As wallBoiling, but with an interfacial area transport equation
for modelling the bubble diameters
The wall boiling tutorials for reactingMultiphaseEulerFoam are:
RAS/wallBoilingPolydisperseTwoGroups:
As wallBoiling, but with an inhomogenous class method population
balance for modelling the bubble diameters
Patch contributed by Juho Peltola, VTT.
Refactored the function for scaling the size group volume fractions to
better handle situations in which their sum drifts away from unity.
Scaling is now turned on by default, and can be turned off in the
solution dictionary for the population balance.
Additional revision and renaming of *Polydisperse tutorials
Patch contributed by Institute of Fluid Dynamics,
Helmholtz-Zentrum Dresden - Rossendorf (HZDR)
This fix also required a generalization of the corresponding base class,
which allows the user to specify the number of daughter particles per
breakup event separately.
Patch contributed by Institute of Fluid Dynamics,
Helmholtz-Zentrum Dresden - Rossendorf (HZDR)
The keyword which selects how the subset over which the function
operates is generated has been renamed to "selectionMode", to make it
more consistent with other parts of the OpenFOAM (e.g., fvOptions). It
can still take the value "all" or "cellZone". A cell zone is now
specified with a "cellZone", again for consistency.
Error messaging has also been overhauled.
Patch contributed by Institute of Fluid Dynamics,
Helmholtz-Zentrum Dresden - Rossendorf (HZDR)
Now for transient simulations "Final" solver settings are required for ALL
equations providing consistency between the solution of velocity, energy,
composition and radiation properties.
However "Final" relaxation factors are no longer required for fields or
equations and if not present the standard value for the variable will be
applied. Given that relaxation factors other than 1 are rarely required for
transient runs and hence the same for all iterations including the final one
this approach provide simpler input while still providing the flexibility to
specify a different value for the final iteration if required. For steady cases
it is usual to execute just 1 outer iteration per time-step for which the
standard relaxation factors are appropriate, and if more than one iteration is
executed it is common to use the same factors for both. In the unlikely event
of requiring different relaxation factors for the final iteration this is still
possible to specify via the now optional "Final" specification.
to avoid the need to evaluate departure functions and simplify evaluation of the
temperature. In general it makes more sense to use and e/Cv based
thermodynamics when solving for internal energy rather than h/Cp and have
convert between the energy forms.
All related tutorials and test cases have also been updated.
An additional layer has been added into the phase system hierarchy which
facilitates the application of phase transfer modelling. These are
models which exchange mass between phases without the thermal coupling
that would be required to represent phase change. They can be thought of
as representation changes; e.g., between two phases representing
different droplet sizes of the same physical fluid.
To facilitate this, the heat transfer phase systems have been modified
and renamed and now both support mass transfer. The two sided version
is only required for derivations which support phase change.
The following changes to case settings have been made:
- The simplest instantiated phase systems have been renamed to
basicTwoPhaseSystem and basicMultiphaseSystem. The
heatAndMomentumTransfer*System entries in constant/phaseProperties files
will need updating accordingly.
- A phaseTransfer sub-model entry will be required in the
constant/phaseProperties file. This can be an empty list.
- The massTransfer switch in thermal phase change cases has been renamed
phaseTransfer, so as not to be confused with the mass transfer models
used by interface composition cases.
This work was supported by Georg Skillas and Zhen Li, at Evonik
Also added tutorial case demonstrating usage. Note that the new drag
models are symmetric and should be used without any blending.
This work was supported by Georg Skillas and Zhen Li, at Evonik
Sub-model blending should be set such that the sum of all the blending
coefficients equals one. If there are three models specified for a phase
pair (e.g., (air in water), (water in air) and (air and water)), then
the sum-to-one constraint is guaranteed by the blending functions.
Frequently, however, the symmetric model ((air and water) in this
example) is omitted. In that case, the blending coefficients should be
selected so that the sum of just the two non-symmetric coefficients
equal one.
In the case of linear blending, this means setting the minimum partially
continuous alpha to one-minus the fully continuous value of the opposite
phase. For example:
blending
{
default
{
type linear;
minFullyContinuousAlpha.air 0.7;
minPartlyContinuousAlpha.air 0.3;
minFullyContinuousAlpha.water 0.7;
minPartlyContinuousAlpha.water 0.3;
}
}
The reactingTwoPhaseEulerFoam and reactingMultiPhaseEulerFoam tutorials
have been modified to adhere to this principle.
Two new phase models have been added as selectable options for
reactingMultiphaseEulerFoam; pureStationaryPhaseModel and
pureStationaryIsothermalPhaseModel. These phases do not store a
velocity and their phase fractions remain constant throughout the
simulation. They are intended for use in modelling static particle beds
and other forms of porous media by means of the existing Euler-Euler
transfer models (drag, heat transfer, etc...).
Note that this functionality has not been extended to
reactingTwoPhaseEulerFoam, or the non-reacting *EulerFoam solvers.
Additional maintenance work has been carried out on the phase model
and phase system structure. The system can now loop over subsets of
phases with specific functionality (moving, multi-component, etc...) in
order to avoid testing for the existence of equations or variables in
the top level solver. The mass transfer handling and it's effect on
per-phase source terms has been refactored to reduce duplication. Const
and non-const access to phase properties has been formalised by renaming
non-const accessors with a "Ref" suffix, which is consistent with other
recent developments to classes including tmp and GeometricField, among
others. More sub-modelling details have been made private in order to
reduce the size of interfaces and improve abstraction.
This work was supported by Zhen Li, at Evonik
The initial set of cases in the test directory are aimed at testing the
reactingEulerFoam populationBalance functionality.
Patch contributed by Institute of Fluid Dynamics, Helmholtz-Zentrum
Dresden - Rossendorf (HZDR) and VTT Technical Research Centre of Finland Ltd.
Integrated with the "tutorials" functionality by CFD Direct Ltd.
This change means that getApplication still works if we have a
controlDict.orig, rather than a controlDict. This allows us to simplify
the scripting of tutorials in which the controlDict is modified.
Some tutorials have had Allrun scripts added in order to run setFields,
which was previously omitted. Others have had nonuniform field files in
the 0 directory replaced by uniform files with .orig extensions.
Now if a <field> file does not exist first the compressed <field>.gz file is
searched for and if that also does not exist the <field>.orig file is searched
for.
This simplifies case setup and run scripts as now setField for example can read
the <field>.orig file directly and generate the <field> file from it which is
then read by the solver. Additionally the cleanCase function used by
foamCleanCase and the Allclean scripts automatically removed <field> files if
there is a corresponding <field>.orig file. So now there is no need for the
Allrun scripts to copy <field>.orig files into <field> or for the Allclean
scripts to explicitly remove them.
Introduced thermalPhaseChangePopulationBalanceTwo- and MultiphaseSystem as
user-selectable phaseSystems which are the first to actually use multiple mass
transfer mechanisms enabled by
commit d3a237f560.
The functionality is demonstrated using the reactingTwoPhaseEulerFoam
wallBoilingPolydisperse tutorial.
Patch contributed by VTT Technical Research Centre of Finland Ltd and Institute
of Fluid Dynamics, Helmholtz-Zentrum Dresden - Rossendorf (HZDR).
Using the noSlip boundary condition for rotating wall in an MRF region
interferes with post-processing by resetting the wall velocity to 0 rather than
preserving the value set by the MRF zone.
Removed possibility for the user to specify a driftRate in the constantDrift
model which is independent of a fvOptions mass source. The driftRate must be
calculated from/be consistent with the mass source in order to yield a particle
number conserving result.
Made calculation of the over-all Sauter mean diameter of an entire population
balance conditional on more than one velocityGroup being present. This diameter
field is for post-processing purposes only and would be redundant in case of one
velocityGroup being used.
Solution control is extended to allow for solution of the population balance
equation at the last PIMPLE loop only, using an optional switch. This can be
beneficial in terms of simulation time as well as coupling between the
population balance based diameter calculation and the rest of the equation
system.
Patch contributed by Institute of Fluid Dynamics, Helmholtz-Zentrum Dresden - Rossendorf
(HZDR) and VTT Technical Research Centre of Finland Ltd.
This patch enables the reactingEulerFoam solvers to simulate polydisperse flow
situations, i.e. flows where the disperse phase is subject to a size
distribution.
The newly added populationBalanceModel class solves the integro-partial
differential population balance equation (PBE) by means of a class method, also
called discrete or sectional method. This approach is based on discretizing the
PBE over its internal coordinate, the particle volume. This yields a set of
transport equations for the number concentration of particles in classes with a
different representative size. These are coupled through their source-terms and
solved in a segregated manner. The implementation is done in a way, that the
total particle number and mass is preserved for coalescence, breakup and drift
(i.e. isothermal growth or phase change) processes, irrespective of the chosen
discretization over the internal coordinate.
A population balance can be split over multiple velocity (temperature) fields,
using the capability of reactingMultiphaseEulerFoam to solve for n momentum
(energy) equations. To a certain degree, this takes into account the dependency
of heat- and momentum transfer on the disperse phase diameter. It is also possible
to define multiple population balances, e.g. bubbles and droplets simultaneously.
The functionality can be switched on by choosing the appropriate phaseSystem
type, e.g. populationBalanceMultiphaseSystem and the newly added diameterModel
class called velocityGroup. To illustrate the use of the functionality, a
bubbleColumnPolydisperse tutorial was added for reactingTwoPhaseEulerFoam and
reactingMultiphaseEulerFoam.
Furthermore, a reactingEulerFoam-specific functionObject called sizeDistribution
was added to allow post-Processing of the size distribution, e.g. to obtain the
number density function in a specific region.
Patch contributed by Institute of Fluid Dynamics, Helmholtz-Zentrum Dresden - Rossendorf
(HZDR) and VTT Technical Research Centre of Finland Ltd.
- Thermal phase change and wall boiling functionality has been generalized to
support two- and multi- phase simulations.
- Thermal phase change now also allows purePhaseModel, which simplifies case setup.
- The phaseSystem templates have been restructured in preparation of multiple
simultaneous mass transfer mechanisms. For example, combination of thermal phase
and inhomogeneous population balance models.
Patch contributed by VTT Technical Research Centre of Finland Ltd and Institute
of Fluid Dynamics, Helmholtz-Zentrum Dresden - Rossendorf (HZDR).
