Sampled sets and streamlines now write all their fields to the same
file. This prevents excessive duplication of the geometry and makes
post-processing tasks more convenient.
"axis" entries are now optional in sampled sets and streamlines. When
omitted, a default entry will be used, which is chosen appropriately for
the coordinate set and the write format. Some combinations are not
supported. For example, a scalar ("x", "y", "z" or "distance") axis
cannot be used to write in the vtk format, as vtk requires 3D locations
with which to associate data. Similarly, a point ("xyz") axis cannot be
used with the gnuplot format, as gnuplot needs a single scalar to
associate with the x-axis.
Streamlines can now write out fields of any type, not just scalars and
vectors, and there is no longer a strict requirement for velocity to be
one of the fields.
Streamlines now output to postProcessing/<functionName>/time/<file> in
the same way as other functions. The additional "sets" subdirectory has
been removed.
The raw set writer now aligns columns correctly.
The handling of segments in coordSet and sampledSet has been
fixed/completed. Segments mean that a coordinate set can represent a
number of contiguous lines, disconnected points, or some combination
thereof. This works in parallel; segments remain contiguous across
processor boundaries. Set writers now only need one write method, as the
previous "writeTracks" functionality is now handled by streamlines
providing the writer with the appropriate segment structure.
Coordinate sets and set writers now have a convenient programmatic
interface. To write a graph of A and B against some coordinate X, in
gnuplot format, we can call the following:
setWriter::New("gnuplot")->write
(
directoryName,
graphName,
coordSet(true, "X", X), // <-- "true" indicates a contiguous
"A", // line, "false" would mean
A, // disconnected points
"B",
B
);
This write function is variadic. It supports any number of
field-name-field pairs, and they can be of any primitive type.
Support for Jplot and Xmgrace formats has been removed. Raw, CSV,
Gnuplot, VTK and Ensight formats are all still available.
The old "graph" functionality has been removed from the code, with the
exception of the randomProcesses library and associated applications
(noise, DNSFoam and boxTurb). The intention is that these should also
eventually be converted to use the setWriters. For now, so that it is
clear that the "graph" functionality is not to be used elsewhere, it has
been moved into a subdirectory of the randomProcesses library.
With this change each functionObject provides the list of fields required so
that the postProcess utility can pre-load them before executing the list of
functionObjects. This provides a more convenient interface than using the
-field or -fields command-line options to postProcess which are now redundant.
The writer class has been renamed setWriter in order to clarify its
usage. The coordSet and setWriter classes have been moved into the
sampling library, as this fits their usage.
Currently these deleted function declarations are still in the private section
of the class declarations but will be moved by hand to the public section over
time as this is too complex to automate reliably.
In early versions of OpenFOAM the scalar limits were simple macro replacements and the
names were capitalized to indicate this. The scalar limits are now static
constants which is a huge improvement on the use of macros and for consistency
the names have been changed to camel-case to indicate this and improve
readability of the code:
GREAT -> great
ROOTGREAT -> rootGreat
VGREAT -> vGreat
ROOTVGREAT -> rootVGreat
SMALL -> small
ROOTSMALL -> rootSmall
VSMALL -> vSmall
ROOTVSMALL -> rootVSmall
The original capitalized are still currently supported but their use is
deprecated.
Now the functionality to write single graph files or log files (vs time)
may be used in the creation of any form of functionObject, not just
those relating to a mesh region.
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.
