PVReaders now support compilation against ParaView version 5.7.0 and
greater. All references to ParaView versions less than 4.0.0 have been
removed.
Based on a patch contributed by CFD Support
These function map to the corresponding functions in the
PhaseThermophysicalTransportModel to allow run-time selection and extensibility
of the phase thermophysical transport.
Provides an abstraction of specie transport to support run-times selectable and
extensible multi-component thermal and specie laminar and turbulent transport.
providing the shear-stress term in the momentum equation for incompressible and
compressible Newtonian, non-Newtonian and visco-elastic laminar flow as well as
Reynolds averaged and large-eddy simulation of turbulent flow.
The general deviatoric shear-stress term provided by the MomentumTransportModels
library is named divDevTau for compressible flow and divDevSigma (sigma =
tau/rho) for incompressible flow, the spherical part of the shear-stress is
assumed to be either included in the pressure or handled separately. The
corresponding stress function sigma is also provided which in the case of
Reynolds stress closure returns the effective Reynolds stress (including the
laminar contribution) or for other Reynolds averaged or large-eddy turbulence
closures returns the modelled Reynolds stress or sub-grid stress respectively.
For visco-elastic flow the sigma function returns the effective total stress
including the visco-elastic and Newtonian contributions.
For thermal flow the heat-flux generated by thermal diffusion is now handled by
the separate ThermophysicalTransportModels library allowing independent run-time
selection of the heat-flux model.
During the development of the MomentumTransportModels library significant effort
has been put into rationalising the components and supporting libraries,
removing redundant code, updating names to provide a more logical, consistent
and extensible interface and aid further development and maintenance. All
solvers and tutorials have been updated correspondingly and backward
compatibility of the input dictionaries provided.
Henry G. Weller
CFD Direct Ltd.
This script allows version numbers to be compared. It is called in the
following way:
foamVersionCompare <version-1> <comparison> <version-2>
The <comparison> argument can be one of; eq (equal-to), lt (less-than),
gt (greater-than), le (less-than-or-equal-to), or ge
(greater-than-or-equal-to). The script returns a successful exit code if
the comparison evaluates as true.
Example usage:
if $WM_PROJECT_DIR/bin/tools/foamVersionCompare 5.4.3 gt 5.5.1
then
echo "5.4.3 IS greater than 5.5.1"
else
echo "5.4.3 is NOT greater than 5.5.1"
fi
This provides an extensible and run-time selectable framework to support complex
energy and specie transport models, in particular multi-component diffusion.
Currently only the Fourier for laminar and eddyDiffusivity for RAS and LES
turbulent flows are provided but the interface is general and the set of models
will be expanded in the near future.
The simplistic energy transport support in compressibleTurbulenceModels has been
abstracted and separated into the new ThermophysicalTransportModels library in
order to provide a more general interface to support complex energy and specie
transport models, in particular multi-component diffusion. Currently only the
Fourier for laminar and eddyDiffusivity for RAS and LES turbulent flows are
provided but the interface is general and the set of models will be expanded in
the near future.
The ThermalDiffusivity and EddyDiffusivity modelling layers remain in
compressibleTurbulenceModels but will be removed shortly and the alphat boundary
conditions will be moved to ThermophysicalTransportModels.
Following the generalisation of the TurbulenceModels library to support
non-Newtonian laminar flow including visco-elasticity and extensible to other
form of non-Newtonian behaviour the name TurbulenceModels is misleading and does
not properly represent how general the OpenFOAM solvers now are. The
TurbulenceModels now provides an interface to momentum transport modelling in
general and the plan is to rename it MomentumTransportModels and in preparation
for this the turbulenceProperties dictionary has been renamed momentumTransport
to properly reflect its new more general purpose.
The old turbulenceProperties name is supported for backward-compatibility.
These provide pressure boundary conditions suitable for use on
boundaries where the flow may reverse or on which the inlet or outlet
state is not known or well defined. The condition takes the following
form:
p = p0 + 0.5*Un*mag(Un)
In the case of exactly normal inlet velocity, this condition sets the
same pressure as the totalPressure condition. The pressure that is set
increases with increasing outlet velocity and decreases with increasing
inlet velocity. This makes it self-limiting and extremely stable in a
number of configurations which were not easily simulated previously. The
condition also does varies smoothly as the flux reverses, which also
aids stability.
The controls of this boundary condition are exactly the same as for the
totalPressure condition. Note, however, that "p0" is not necessarily the
total pressure any more. It is, in general, a reference pressure.
An example usage is as follows:
sides
{
type entrainmentPressure;
p0 100;
}
Additional flexibility for handling of field arguments has been extended
to dictionary lists of field settings, as well as word lists of field
names. This means that the following syntax is now supported:
postProcess -func "fieldAverage(p, U { prime2Mean on; }, T)"
postProcess -func "fieldAverage(fields=(p U { prime2Mean on; } T))"
Function object argument parsing now takes all "field", "fields" and
"objects" arguments and combines them into a single list of
fields/objects that the function should operate on. This means that the
following postProcess executions are now all equivalent and function as
expected:
postProcess -func "
flowRatePatch
(
name=outlet,
phi,
alphaRhoPhi.air,
alphaRhoPhi.particles
)"
postProcess -func "
flowRatePatch
(
name=outlet,
fields=(phi alphaRhoPhi.air alphaRhoPhi.particles)
)"
postProcess -func "
flowRatePatch
(
name=outlet,
objects=(phi),
alphaRhoPhi.air,
field=alphaRhoPhi.particles
)"
As are the following:
postProcess -func "mag(U.air)"
postProcess -func "mag(field=U.air)"
renaming the legacy keywords
RASModel -> model
LESModel -> model
laminarModel -> model
which is simpler and clear within the context in which they are specified, e.g.
RAS
{
model kOmegaSST;
turbulence on;
printCoeffs on;
}
rather than
RAS
{
RASModel kOmegaSST;
turbulence on;
printCoeffs on;
}
The old keywords are supported for backward compatibility.
The ability to specify the file name of the turbulenceProperties dictionary
during construction was added to support multi-phases but now that the handling
of the phase name extension has been completely rationalised and standardised
this complexity and code clutter is no longer used, needed or appropriate.
This significant improvement is flexibility of SemiImplicitSource required a
generalisation of the source specification syntax and all tutorials have been
updated accordingly.
Description
Semi-implicit source, described using an input dictionary. The injection
rate coefficients are specified as pairs of Su-Sp coefficients, i.e.
\f[
S(x) = S_u + S_p x
\f]
where
\vartable
S(x) | net source for field 'x'
S_u | explicit source contribution
S_p | linearised implicit contribution
\endvartable
Example tabulated heat source specification for internal energy:
\verbatim
volumeMode absolute; // specific
sources
{
e
{
explicit table ((0 0) (1.5 $power));
implicit 0;
}
}
\endverbatim
Example coded heat source specification for enthalpy:
\verbatim
volumeMode absolute; // specific
sources
{
h
{
explicit
{
type coded;
name heatInjection;
code
#{
// Power amplitude
const scalar powerAmplitude = 1000;
// x is the current time
return mag(powerAmplitude*sin(x));
#};
}
implicit 0;
}
}
\endverbatim
All of these sets will now take either "set" as the input entry, or
"cellSet"/"faceSet"/"pointSet" as appropriate. Previously cell and point
only accepted the "set" keyword whilst face only took "faceSet".
This is a topoSetSource which selects faces based on the adjacent cell
centres spanning a given plane. The plane is defined by a point and
normal vector.
Additionally, an include entry can be specified. When omitted or set to
"all", then all faces that meet the criteria are included in the set. When
set to "closest", just the faces that belong to the closest contiguous
region to the plane point are included. This latter setting is useful when
defining face zones through channels on which the flow rate is to be
computed, as it keeps the set local to a single channel.
An example usage (in system/topoSetDict) is as follows:
actions
(
{
name f0;
type faceZoneSet;
action new;
source planeToFaceZone;
sourceInfo
{
point (0 0 4);
normal (1 0 0.2);
include closest;
}
}
);
This would then allow the flow rate through the created face zone to be
accurately reported by the following command:
postProcess -func "flowRateFaceZone(name=f0,field=phi)"
