terms of the local barycentric coordinates of the current tetrahedron,
rather than the global coordinate system.
Barycentric tracking works on any mesh, irrespective of mesh quality.
Particles do not get "lost", and tracking does not require ad-hoc
"corrections" or "rescues" to function robustly, because the calculation
of particle-face intersections is unambiguous and reproducible, even at
small angles of incidence.
Each particle position is defined by topology (i.e. the decomposed tet
cell it is in) and geometry (i.e. where it is in the cell). No search
operations are needed on restart or reconstruct, unlike when particle
positions are stored in the global coordinate system.
The particle positions file now contains particles' local coordinates
and topology, rather than the global coordinates and cell. This change
to the output format is not backwards compatible. Existing cases with
Lagrangian data will not restart, but they will still run from time
zero without any modification. This change was necessary in order to
guarantee that the loaded particle is valid, and therefore
fundamentally prevent "loss" and "search-failure" type bugs (e.g.,
2517, 2442, 2286, 1836, 1461, 1341, 1097).
The tracking functions have also been converted to function in terms
of displacement, rather than end position. This helps remove floating
point error issues, particularly towards the end of a tracking step.
Wall bounded streamlines have been removed. The implementation proved
incompatible with the new tracking algorithm. ParaView has a surface
LIC plugin which provides equivalent, or better, functionality.
Additionally, bug report <https://bugs.openfoam.org/view.php?id=2517>
is resolved by this change.
except turbulence and lagrangian which will also be updated shortly.
For example in the nonNewtonianIcoFoam offsetCylinder tutorial the viscosity
model coefficients may be specified in the corresponding "<type>Coeffs"
sub-dictionary:
transportModel CrossPowerLaw;
CrossPowerLawCoeffs
{
nu0 [0 2 -1 0 0 0 0] 0.01;
nuInf [0 2 -1 0 0 0 0] 10;
m [0 0 1 0 0 0 0] 0.4;
n [0 0 0 0 0 0 0] 3;
}
BirdCarreauCoeffs
{
nu0 [0 2 -1 0 0 0 0] 1e-06;
nuInf [0 2 -1 0 0 0 0] 1e-06;
k [0 0 1 0 0 0 0] 0;
n [0 0 0 0 0 0 0] 1;
}
which allows a quick change between models, or using the simpler
transportModel CrossPowerLaw;
nu0 [0 2 -1 0 0 0 0] 0.01;
nuInf [0 2 -1 0 0 0 0] 10;
m [0 0 1 0 0 0 0] 0.4;
n [0 0 0 0 0 0 0] 3;
if quick switching between models is not required.
To support this more convenient parameter specification the inconsistent
specification of seedSampleSet in the streamLine and wallBoundedStreamLine
functionObjects had to be corrected from
// Seeding method.
seedSampleSet uniform; //cloud; //triSurfaceMeshPointSet;
uniformCoeffs
{
type uniform;
axis x; //distance;
// Note: tracks slightly offset so as not to be on a face
start (-1.001 -0.05 0.0011);
end (-1.001 -0.05 1.0011);
nPoints 20;
}
to the simpler
// Seeding method.
seedSampleSet
{
type uniform;
axis x; //distance;
// Note: tracks slightly offset so as not to be on a face
start (-1.001 -0.05 0.0011);
end (-1.001 -0.05 1.0011);
nPoints 20;
}
which also support the "<type>Coeffs" form
// Seeding method.
seedSampleSet
{
type uniform;
uniformCoeffs
{
axis x; //distance;
// Note: tracks slightly offset so as not to be on a face
start (-1.001 -0.05 0.0011);
end (-1.001 -0.05 1.0011);
nPoints 20;
}
}
Replaced the 'postProcess' argument to the 'write' and 'execute'
functions with the single static member 'postProcess' in the
functionObject base-class.
with the more general and flexible 'postProcess' utility and '-postProcess' solver option
Rationale
---------
Both the 'postProcess' utility and '-postProcess' solver option use the
same extensive set of functionObjects available for data-processing
during the run avoiding the substantial code duplication necessary for
the 'foamCalc' and 'postCalc' utilities and simplifying maintenance.
Additionally consistency is guaranteed between solver data processing
and post-processing.
The functionObjects have been substantially re-written and generalized
to simplify development and encourage contribution.
Configuration
-------------
An extensive set of simple functionObject configuration files are
provided in
OpenFOAM-dev/etc/caseDicts/postProcessing
and more will be added in the future. These can either be copied into
'<case>/system' directory and included into the 'controlDict.functions'
sub-dictionary or included directly from 'etc/caseDicts/postProcessing'
using the '#includeEtc' directive or the new and more convenient
'#includeFunc' directive which searches the
'<etc>/caseDicts/postProcessing' directories for the selected
functionObject, e.g.
functions
{
#includeFunc Q
#includeFunc Lambda2
}
'#includeFunc' first searches the '<case>/system' directory in case
there is a local configuration.
Description of #includeFunc
---------------------------
Specify a functionObject dictionary file to include, expects the
functionObject name to follow (without quotes).
Search for functionObject dictionary file in
user/group/shipped directories.
The search scheme allows for version-specific and
version-independent files using the following hierarchy:
- \b user settings:
- ~/.OpenFOAM/\<VERSION\>/caseDicts/postProcessing
- ~/.OpenFOAM/caseDicts/postProcessing
- \b group (site) settings (when $WM_PROJECT_SITE is set):
- $WM_PROJECT_SITE/\<VERSION\>/caseDicts/postProcessing
- $WM_PROJECT_SITE/caseDicts/postProcessing
- \b group (site) settings (when $WM_PROJECT_SITE is not set):
- $WM_PROJECT_INST_DIR/site/\<VERSION\>/caseDicts/postProcessing
- $WM_PROJECT_INST_DIR/site/caseDicts/postProcessing
- \b other (shipped) settings:
- $WM_PROJECT_DIR/etc/caseDicts/postProcessing
An example of the \c \#includeFunc directive:
\verbatim
#includeFunc <funcName>
\endverbatim
postProcess
-----------
The 'postProcess' utility and '-postProcess' solver option provide the
same set of controls to execute functionObjects after the run either by
reading a specified set of fields to process in the case of
'postProcess' or by reading all fields and models required to start the
run in the case of '-postProcess' for each selected time:
postProcess -help
Usage: postProcess [OPTIONS]
options:
-case <dir> specify alternate case directory, default is the cwd
-constant include the 'constant/' dir in the times list
-dict <file> read control dictionary from specified location
-field <name> specify the name of the field to be processed, e.g. U
-fields <list> specify a list of fields to be processed, e.g. '(U T p)' -
regular expressions not currently supported
-func <name> specify the name of the functionObject to execute, e.g. Q
-funcs <list> specify the names of the functionObjects to execute, e.g.
'(Q div(U))'
-latestTime select the latest time
-newTimes select the new times
-noFunctionObjects
do not execute functionObjects
-noZero exclude the '0/' dir from the times list, has precedence
over the -withZero option
-parallel run in parallel
-region <name> specify alternative mesh region
-roots <(dir1 .. dirN)>
slave root directories for distributed running
-time <ranges> comma-separated time ranges - eg, ':10,20,40:70,1000:'
-srcDoc display source code in browser
-doc display application documentation in browser
-help print the usage
pimpleFoam -postProcess -help
Usage: pimpleFoam [OPTIONS]
options:
-case <dir> specify alternate case directory, default is the cwd
-constant include the 'constant/' dir in the times list
-dict <file> read control dictionary from specified location
-field <name> specify the name of the field to be processed, e.g. U
-fields <list> specify a list of fields to be processed, e.g. '(U T p)' -
regular expressions not currently supported
-func <name> specify the name of the functionObject to execute, e.g. Q
-funcs <list> specify the names of the functionObjects to execute, e.g.
'(Q div(U))'
-latestTime select the latest time
-newTimes select the new times
-noFunctionObjects
do not execute functionObjects
-noZero exclude the '0/' dir from the times list, has precedence
over the -withZero option
-parallel run in parallel
-postProcess Execute functionObjects only
-region <name> specify alternative mesh region
-roots <(dir1 .. dirN)>
slave root directories for distributed running
-time <ranges> comma-separated time ranges - eg, ':10,20,40:70,1000:'
-srcDoc display source code in browser
-doc display application documentation in browser
-help print the usage
The functionObjects to execute may be specified on the command-line
using the '-func' option for a single functionObject or '-funcs' for a
list, e.g.
postProcess -func Q
postProcess -funcs '(div(U) div(phi))'
In the case of 'Q' the default field to process is 'U' which is
specified in and read from the configuration file but this may be
overridden thus:
postProcess -func 'Q(Ua)'
as is done in the example above to calculate the two forms of the divergence of
the velocity field. Additional fields which the functionObjects may depend on
can be specified using the '-field' or '-fields' options.
The 'postProcess' utility can only be used to execute functionObjects which
process fields present in the time directories. However, functionObjects which
depend on fields obtained from models, e.g. properties derived from turbulence
models can be executed using the '-postProcess' of the appropriate solver, e.g.
pisoFoam -postProcess -func PecletNo
or
sonicFoam -postProcess -func MachNo
In this case all required fields will have already been read so the '-field' or
'-fields' options are not be needed.
Henry G. Weller
CFD Direct Ltd.
