For a set to zone conversion the name of the zone is now specified with the
'zone' keyword.
For a patch to set conversion the name of the patch is now specified with the
'patch' keyword.
Backward-compatibility is supported for both these changes.
Additionally the file name of a searchableSurface file is specified with the
'file' keyword. This should be 'surface' but that keyword is currently and
confusingly used for the surface type rather than name and this cannot be
changed conveniently while maintaining backward compatibility.
and only needed if there is a name clash between entries in the source
specification and the set specification, e.g. "name":
{
name rotorCells;
type cellSet;
action new;
source zoneToCell;
sourceInfo
{
name cylinder;
}
}
Description
A topoSetSource to select patch faces according to the flux direction.
Usage
Example topoSetDict to generate faceSets for inflow and outflow faces
on the outlet patch:
\verbatim
actions
(
{
action new;
type faceSet;
name inflow;
source patchFluxToFace;
sourceInfo
{
field phi;
patch outlet;
inflow true;
}
}
{
action new;
type faceSet;
name outflow;
source patchFluxToFace;
sourceInfo
{
field phi;
patch outlet;
inflow false;
}
}
);
\endverbatim
topoSet is a more flexible and extensible replacement for setSet using standard
OpenFOAM dictionary input format rather than the limited command-line input
format developed specifically for setSet. This replacement allows for the
removal of a significant amount of code simplifying maintenance and the addition
of more topoSet sources.
The icx and icpx Intel compilers are selected by
WM_COMPILER=Icx
These compilers are based on the Clang front-end and hence the configuration
files are based on and nearly identical to those for Clang.
Support for the new OneAPI compilers replaces the now deprecated Intel icc, icpc
compilers.
Removed the combustion/reactingFoam/Lagrangian/counterFlowFlame2DLTS
case as it was originally a consistency check between reactingFoam and
reactingParcelFoam. It is not necessary now these solvers have been
combined.
Removed an unused fvModels file in the
reactingFoam/Lagrangian/simplifiedSiwek tutorial.
Packaged function objects can now be deployed equally effectively by
(a) using a locally edited copy of the configuration file, or by
(b) passing parameters as arguments to the global configuration file.
For example, to post-process the pressure field "p" at a single location
"(1 2 3)", the user could first copy the "probes" packaged function
object file to their system directory by calling "foamGet probes". They
could then edit the file to contain the following entries:
points ((1 2 3));
field p;
The function object can then be executed by the postProcess application:
postProcess -func probes
Or it can be called at run-time, by including from within the functions
section of the system/controlDict file:
#includeFunc probes
Alternatively, the field and points parameters could be passed as
arguments either to the postProcess application by calling:
postProcess -func "probes(points=((1 2 3)), p)"
Or by using the #includeFunc directive:
#includeFunc probes(points=((1 2 3)), p)
In both cases, mandatory parameters that must be either edited or
provided as arguments are denoted in the configuration files with
angle-brackets, e.g.:
points (<points>);
Many of the packaged function objects have been split up to make them
more specific to a particular use-case. For example, the "surfaces"
function has been split up into separate functions for each surface
type; "cutPlaneSurface", "isoSurface", and "patchSurface". This
splitting means that the packaged functions now only contain one set of
relevant parameters so, unlike previously, they now work effectively
with their parameters passed as arguments. To ensure correct usage, all
case-dependent parameters are considered mandatory.
For example, the "streamlines" packaged function object has been split
into specific versions; "streamlinesSphere", "streamlinesLine",
"streamlinesPatch" and "streamlinesPoints". The name ending denotes the
seeding method. So, the following command creates ten streamlines with
starting points randomly seeded within a sphere with a specified centre
and radius:
postProcess -func "streamlinesSphere(nPoints=10, centre=(0 0 0), radius=1)"
The equivalent #includeFunc approach would be:
#includeFunc streamlinesSphere(nPoints=10, centre=(0 0 0), radius=1)
When passing parameters as arguments, error messages report accurately
which mandatory parameters are missing and provide instructions to
correct the format of the input. For example, if "postProcess -func
graphUniform" is called, then the code prints the following error message:
--> FOAM FATAL IO ERROR:
Essential value for keyword 'start' not set
Essential value for keyword 'end' not set
Essential value for keyword 'nPoints' not set
Essential value for keyword 'fields' not set
In function entry:
graphUniform
In command:
postProcess -func graphUniform
The function entry should be:
graphUniform(start = <point>, end = <point>, nPoints = <number>, fields = (<fieldNames>))
file: controlDict/functions/graphUniform from line 15 to line 25.
As always, a full list of all packaged function objects can be obtained
by running "postProcess -list", and a description of each function can
be obtained by calling "foamInfo <functionName>". An example case has
been added at "test/postProcessing/channel" which executes almost all
packaged function objects using both postProcess and #includeFunc. This
serves both as an example of syntax and as a unit test for maintenance.
The fieldsExpression function has been generalised to work with a
general operator. Existing functions "add" and "subtract" have been made
to use this system, and two new operations, "multiply" and "divide",
have been added.
The functions can now handle multiple types in both input and output. A
multiply (outer product) operation on two vectors and a scalar will
result in a tensor. If the operation chain is not supported (e.g.,
division by a vector) then a warning will be generated.
In addition, a "uniform" function has been added, which will create a
uniform geometric field of a given type with specified dimensions and
calculated boundary conditions. This is mostly useful for testing
purposes and for conveniently creating simple input fields for the
operation functions described above. The function can be called by
postProcess as follows:
postProcess -func "uniform(fieldType=volScalarField, name=length, dimensions=[m], value=2)"
A number of changes have been made to the surfaceFieldValue and
volFieldValue function objects to improve their usability and
performance, and to extend them so that similar duplicate functionality
elsewhere in OpenFOAM can be removed.
Weighted operations have been removed. Weighting for averages and sums
is now triggered simply by the existence of the "weightField" or
"weightFields" entry. Multiple weight fields are now supported in both
functions.
The distinction between oriented and non-oriented fields has been
removed from surfaceFieldValue. There is now just a single list of
fields which are operated on. Instead of oriented fields, an
"orientedSum" operation has been added, which should be used for
flowRate calculations and other similar operations on fluxes.
Operations minMag and maxMag have been added to both functions, to
calculate the minimum and maximum field magnitudes respectively. The min
and max operations are performed component-wise, as was the case
previously.
In volFieldValue, minMag and maxMag (and min and mag operations when
applied to scalar fields) will report the location, cell and processor
of the maximum or minimum value. There is also a "writeLocation" option
which if set will write this location information into the output file.
The fieldMinMax function has been made obsolete by this change, and has
therefore been removed.
surfaceFieldValue now operates in parallel without accumulating the
entire surface on the master processor for calculation of the operation.
Collecting the entire surface on the master processor is now only done
if the surface itself is to be written out.
For example, 'foamInfo RosinRammler' includes in the output:
Model
This appears to be the 'RosinRammler' model of the 'distributionModels' family.
The models in the 'distributionModels' family are:
+ exponential
+ fixedValue
+ general
+ massRosinRammler
+ multiNormal
+ normal
+ RosinRammler
+ uniform
With this change both of the following commands are equivalent:
topoSet -region air -dict topoSetDict1
topoSet -region air -dict system/air/topoSetDict1
I.e., if the system/<regionName> path is not specified then it is
assumed.
to avoid further confusion from users migrating from very old OpenFOAM versions.
The surfaceFeatureExtract utility has been superseded and replaced by by the
more general surfaceFeatures utility.
surfaceFeatures reads a surfaceFeaturesDict input file with a much
simpler, more convenient format. Example surfaceFeaturesDict files
can be found in the tutorial and template cases, e.g. located as
follows:
find \$FOAM_TUTORIALS -name surfaceFeaturesDict
find \$FOAM_ETC -name surfaceFeaturesDict
With this change both
blockMesh -dict fineBlockMeshDict
blockMesh -dict system/fineBlockMeshDict
are supported, if the system/ path is not specified it is assumed
Settings for the particleTracks utility are now specified in
system/particleTracksDict. Correspondingly, settings for
steadyParticleTracks are now specified in
system/steadyParticleTracksDict.
The -dict option is now handled correctly and consistently across all
applications with -dict options. The logic associated with doing so has
been centralised.
If a relative path is given to the -dict option, then it is assumed to
be relative to the case directory. If an absolute path is given, then it
is used without reference to the case directory. In both cases, if the
path is found to be a directory, then the standard dictionary name is
appended to the path.
Resolves bug report http://bugs.openfoam.org/view.php?id=3692
The patchType override logic has been simplified and made consistent
between fv, fvs and point patch fields. The "constraintType" attribute
has been removed from point fields as it was not being used.
This change fixes failures that occur with the mapping of fields with
patchType overrides. It fixes a crash that previously occurred when
redistributing patch fields with patchType overrides. It also makes
decomposition correctly maintain patchType overrides on cyclics when
those cyclics are separated and become processorCyclics.
These fixes have been achieved by removing the patchType override data
from the fv and point patches. Whether or not the field overrides the
underlying patchType constraint is now determined on the fly from the
patch and field names and what is available on the field run-time
selection table.
This is the 2006 version of Wilcox's k-omega RAS turbulence model which has some
similarities in formulation and behaviour to the k-omega-SST model but is much
simpler and cleaner. This model is likely to perform just as well as the
k-omega-SST model for a wide range of engineering cases.
Description
Standard (2006) high Reynolds-number k-omega turbulence model for
incompressible and compressible flows.
References:
\verbatim
Wilcox, D. C. (2006).
Turbulence modeling for CFD, 3rd edition
La Canada, CA: DCW industries, Inc.
Wilcox, D. C. (2008).
Formulation of the kw turbulence model revisited.
AIAA journal, 46(11), 2823-2838.
\endverbatim
The default model coefficients are
\verbatim
kOmega2006Coeffs
{
Cmu 0.09;
beta0 0.0708;
gamma 0.52;
Clim 0.875;
alphak 0.6;
alphaOmega 0.5;
}
\endverbatim
