Removed all the special handling for awkward particles from the
nearWallFields function object. The version 5+ tracking already handles
this more robustly.
Resolves bug-report https://bugs.openfoam.org/view.php?id=2728
Two boundary conditions for the modelling of semi-permeable baffles have
been added. These baffles are permeable to a number of species within
the flow, and are impermeable to others. The flux of a given species is
calculated as a constant multipled by the drop in mass fraction across
the baffle.
The species mass-fraction condition requires the transfer constant and
the name of the patch on the other side of the baffle:
boundaryField
{
// ...
membraneA
{
type semiPermeableBaffleMassFraction;
samplePatch membranePipe;
c 0.1;
value uniform 0;
}
membraneB
{
type semiPermeableBaffleMassFraction;
samplePatch membraneSleeve;
c 0.1;
value uniform 1;
}
}
If the value of c is omitted, or set to zero, then the patch is
considered impermeable to the species in question. The samplePatch entry
can also be omitted in this case.
The velocity condition does not require any special input:
boundaryField
{
// ...
membraneA
{
type semiPermeableBaffleVelocity;
value uniform (0 0 0);
}
membraneB
{
type semiPermeableBaffleVelocity;
value uniform (0 0 0);
}
}
These two boundary conditions must be used in conjunction, and the
mass-fraction condition must be applied to all species in the
simulation. The calculation will fail with an error message if either is
used in isolation.
A tutorial, combustion/reactingFoam/RAS/membrane, has been added which
demonstrates this transfer process.
This work was done with support from Stefan Lipp, at BASF.
The forces function object, when specified with a full coordinate
system, previously wrote forces and moments out in the following format:
time-0 forces-0 moments-0
time-0 localForces-0 localMoments-0
time-1 forces-1 moments-1
time-1 localForces-1 localMoments-1
# etc ...
There are two rows of values per time. This complicates the definition
of the table and means that filtering has to be done before the data
series can be visualised. The format has now been changed to the
following form:
time-0 forces-0 moments-0 localForces-0 localMoments-0
time-1 forces-1 moments-1 localForces-1 localMoments-1
# etc ...
There is one row per time, and each column is therefore a continuous
series of one variable that can be plotted.
To disable face correspondence checking set
checkFaceCorrespondence off;
in blockMeshDict. This is necessary in the rare cases where adjacent block
faces do not need to correspond because they are geometrically collapsed,
e.g. to form a pole/axis.
Resolves bug-report https://bugs.openfoam.org/view.php?id=2711
A patch can now be assigned to a baffle surface. This assignment will
take precedence over any face-zones.
surfaceConformation
{
locationInMesh (0 0 0);
geometryToConformTo
{
disk
{
featureMethod extractFeatures;
includedAngle 120;
meshableSide both; // <-- baffle
patchInfo
{
type wall;
inGroups (walls);
}
}
// ...
}
}
Foamy surface conformation entries have a "meshableSide" entry which
controls which side of the surface is to be meshed. Typically this is
set "inside" for boundaries and "both" for baffles. A sub-region's
default entry is now taken from it's parent, rather than a specific
value (it was "inside"). This is consistent with how other entries are
handled.
surfaceConformation
{
locationInMesh (0 0 0);
geometryToConformTo
{
baffle
{
featureMethod extractFeatures;
includedAngle 120;
meshableSide both; // <-- per-surface setting
regions
{
disk
{
meshableSide both; // <-- per-region setting*
// *in this example, this entry is not needed, as it
// is taken from the per-surface setting above
}
}
}
// ...
}
}
Specifying default fields for complex and multi-phase cases is simplified and
generalized by using wildcards to select sets of related field names, e.g.
defaultFields (p p_rgh U "U\..*" T "T\..*" "alpha\..*");
selects the velocity, temperature and phase-fraction fields of all phases in
addition to the pressure fields.
The default patch types specified in the new defaultPatchTypes entry of the
etc paraFoam configuration dictionaries:
defaultPatchTypes (patch wall);
Wildcards are supported, for example to specify that all patches loaded simply set
defaultPatchTypes to
defaultPatchTypes (".*");
The new default paraFoam configuration is in the files OpenFOAM-dev/etc/paraFoam
containing the entry
defaultFields (U p p_rgh T alpha.water alpha.air);
specifying the set of fields which are loaded by default if available. This
setting maybe overridden by providing additional paraFoam configuration files in
any of the OpenFOAM etc directories searched, listed using
foamEtcFile -list
e.g.
~/.OpenFOAM/dev
~/.OpenFOAM
~/OpenFOAM/site/dev
~/OpenFOAM/site
~/OpenFOAM/OpenFOAM-dev/etc
The new configurable set of default fields loaded replaces the original hard-coded default of
"p" and "U" and is much more convenient for current OpenFOAM usage.
A wavePressure boundary condition has been added, and the Airy-type wave
models have been extended to generate the unsteady pressure field. This
provides another option for specifying wave motion at a boundary.
If a waveVelocity condition is used in isolation, then any outlet flow
will be extrapolated and scaled to match the required flow rate. This is
similar to how a flowRateOutletVelocity condition works.
0/U:
<patchName>
{
type waveVelocity;
// wave parameters ...
}
0/p_rgh:
<patchName>
{
type fixedFluxPressure;
}
If a waveVelocity is used in conjunction with the new wavePressure
condition, then one will set the value and the other the gradient, as
appropriate for the direction of the flow.
0/U:
<patchName>
{
type waveVelocity;
// wave parameters ...
p p_rgh;
}
0/p_rgh:
<patchName>
{
type wavePressure;
}
This new pressure-velocity formulation is less stable, but generates
more accurate waveforms on patches where the velocity reverses. It is
also necessary for sub-surface cases where fixing the velocity around
the entire domain generates a continuity error.
This work was supported by Alice Gillespie, on behalf of M3 Wave
