This change makes multiphaseEuler more consistent with other modules and
makes its sub-libraries less inter-dependent. Some left-over references
to multiphaseEulerFoam have also been removed.
Population balance size-group fraction 'f<index>.<phase>' fields are now
read from an 'fDefault.<phase>' field if they are not provided
explicitly. This is the same process as is applied to species fractions
or fvDOM rays. The sum-of-fs field 'f.<phase>' is no longer required.
The value of a fraction field and its boundary conditions must now be
specified in the corresponding field file. Value entries are no longer
given in the size group dictionaries in the constant/phaseProperties
file, and an error message will be generated if a value entry is found.
The fraction fields are now numbered programatically, rather than being
named. So, the size-group dictionaries do not require a name any more.
All of the above is also true for any 'kappa<index>.<phase>' fields that
are constructed and solved for as part of a fractal shape model.
The following is an example of a specification of a population balance
with two phases in it:
populationBalances (bubbles);
air1
{
type pureIsothermalPhaseModel;
diameterModel velocityGroup;
velocityGroupCoeffs
{
populationBalance bubbles;
shapeModel spherical;
sizeGroups
(
{ dSph 1e-3; } // Size-group #0: Fraction field f0.air1
{ dSph 2e-3; } // ...
{ dSph 3e-3; }
{ dSph 4e-3; }
{ dSph 5e-3; }
);
}
residualAlpha 1e-6;
}
air2
{
type pureIsothermalPhaseModel;
diameterModel velocityGroup;
velocityGroupCoeffs
{
populationBalance bubbles;
shapeModel spherical;
sizeGroups
(
{ dSph 6e-3; } // Size-group #5: Fraction field f5.air2
{ dSph 7e-3; } // ...
{ dSph 8e-3; }
{ dSph 9e-3; }
{ dSph 10e-3; }
{ dSph 11e-3; }
{ dSph 12e-3; }
);
}
residualAlpha 1e-6;
}
Previously a fraction field was constructed automatically using the
boundary condition types from the sum-of-fs field, and the value of both
the internal and boundary field was then overridden by the value setting
provided for the size-group. This procedure doesn't generalise to
boundary conditions other than basic types that store no additional
data, like zeroGradient and fixedValue. More complex boundary conditions
such as inletOutlet and uniformFixedValue are incompatible with this
approach.
This is arguably less convenient than the previous specification, where
the sizes and fractions appeared together in a table-like list in the
sizeGroups entry. In the event that a substantial proportion of the
size-groups have a non-zero initial fraction, writing out all the field
files manually is extremely tedious. To mitigate this somewhat, a
packaged function has been added to initialise the fields given a file
containing a size distribution (see the pipeBend tutorial for an example
of its usage). This function has the same limitations as the previous
code in that it requires all boundary conditions to be default
constructable.
Ultimately, the "correct" fix for the issue of how to set the boundary
conditions conveniently is to create customised inlet-outlet boundary
conditions that determine their field's position within the population
balance and evaluate a distribution to determine the appropriate inlet
value. This work is pending funding.
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
)
Following the addition of the new moments functionObject, all related
functionality was removed from sizeDistribution.
In its revised version, sizeDistribution allows for different kinds of
weighted region averaging in case of field-dependent representative
particle properties.
A packaged function has also been added to allow for command line solver
post-processing.
For example, the following function object specification returns the
volume-based number density function:
numberDensity
{
type sizeDistribution;
libs ("libmultiphaseEulerFoamFunctionObjects.so");
writeControl writeTime;
populationBalance bubbles;
functionType numberDensity;
coordinateType volume;
setFormat raw;
}
The same can be achieved using a packaged function:
#includeFunc sizeDistribution
(
populationBalance=bubbles,
functionType=numberDensity,
coordinateType=volume,
funcName=numberDensity
)
Or on the command line:
multiphaseEulerFoam -postProcess -func "
sizeDistribution
(
populationBalance=bubbles,
functionType=numberDensity,
coordinateType=volume,
funcName=numberDensity
)"
Patch contributed by Institute of Fluid Dynamics,
Helmholtz-Zentrum Dresden - Rossendorf (HZDR)
This function calculates integral (integer moments) or mean properties
(mean, variance, standard deviation) of a size distribution computed with
multiphaseEulerFoam. It has to be run with multiphaseEulerFoam, either
at run-time or with -postProcess. It will not work with the postProcess
utility.
The following function object specification for example returns the first
moment of the volume-based number density function which is equivalent to
the phase fraction of the particulate phase:
moments
{
type moments;
libs ("libmultiphaseEulerFoamFunctionObjects.so");
executeControl timeStep;
writeControl writeTime;
populationBalance bubbles;
momentType integerMoment;
coordinateType volume;
order 1;
}
The same can be achieved using a packaged function:
#includeFunc moments
(
populationBalance=bubbles,
momentType=integerMoment,
coordinateType=volume,
order=1,
funcName=moments
)
Or on the command line:
multiphaseEulerFoam -postProcess -func "
moments
(
populationBalance=bubbles,
momentType=integerMoment,
coordinateType=volume,
order=1,
funcName=moments
)"
Patch contributed by Institute of Fluid Dynamics,
Helmholtz-Zentrum Dresden - Rossendorf (HZDR)
