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.
In most boundary conditions, fvOptions etc. required and optional fields
to be looked-up from the objectRegistry are selected by setting the
keyword corresponding to the standard field name in the BC etc. to the
appropriate name in the objectRegistry. Usually a default is provided
with sets the field name to the keyword name, e.g. in the
totalPressureFvPatchScalarField the velocity is selected by setting the
keyword 'U' to the appropriate name which defaults to 'U':
Property | Description | Required | Default value
U | velocity field name | no | U
phi | flux field name | no | phi
.
.
.
However, in some BCs and functionObjects and many fvOptions another
convention is used in which the field name keyword is appended by 'Name'
e.g.
Property | Description | Required | Default value
pName | pressure field name | no | p
UName | velocity field name | no | U
This difference in convention is unnecessary and confusing, hinders code
and dictionary reuse and complicates code maintenance. In this commit
the appended 'Name' is removed from the field selection keywords
standardizing OpenFOAM on the first convention above.
This changes simplifies the specification of functionObjects in
controlDict and is consistent with the 'libs' option in controlDict to
load special solver libraries.
Support for the old 'functionObjectLibs' name is supported for backward compatibility.
- Avoids the need for the 'OutputFilterFunctionObject' wrapper
- Time-control for execution and writing is now provided by the
'timeControlFunctionObject' which instantiates the processing
'functionObject' and controls its operation.
- Alternative time-control functionObjects can now be written and
selected at run-time without the need to compile wrapped version of
EVERY existing functionObject which would have been required in the
old structure.
- The separation of 'execute' and 'write' functions is now formalized in the
'functionObject' base-class and all derived classes implement the
two functions.
- Unnecessary implementations of functions with appropriate defaults
in the 'functionObject' base-class have been removed reducing
clutter and simplifying implementation of new functionObjects.
- The 'coded' 'functionObject' has also been updated, simplified and tested.
- Further simplification is now possible by creating some general
intermediate classes derived from 'functionObject'.
to have the prefix 'write' rather than 'output'
So outputTime() -> writeTime()
but 'outputTime()' is still supported for backward-compatibility.
Also removed the redundant secondary-writing functionality from Time
which has been superseded by the 'writeRegisteredObject' functionObject.
for consistency with the time controls in controlDict and to avoid
unnecessary confusion. All code and tutorials have been updated.
The old names 'outputControl' and 'outputInterval' are but supported for
backward compatibility but deprecated.
See http://www.openfoam.org/mantisbt/view.php?id=2076
- .org is the file extension for emacs org-mode as well
- .orig is more to the point (.org isn't always recognized as "original")
- .original is too long, although more consistent with the convention
of source code file naming
Update script contributed by Bruno Santos
BUG: cyclicACMI: make conservative and remove faceAreas0
Need to review cyclicACMI patch non-overlap values
- values here preserve initial values only
- snGrad - used?
- wall functions - no longer call updateCoeffs with ACMI weights (?)
See merge request !46
RunFunctions: Added "isTest()" argument parsing function
tutorials: Updated Allrun scripts to propagate the "-test" option
tutorials: Removed the lower Alltest scripts and updated the Allrun to
use the "isTest()" function to handle test-specific operation
The boundary conditions of HbyA are now constrained by the new "constrainHbyA"
function which applies the velocity boundary values for patches for which the
velocity cannot be modified by assignment and pressure extrapolation is
not specified via the new
"fixedFluxExtrapolatedPressureFvPatchScalarField".
The new function "constrainPressure" sets the pressure gradient
appropriately for "fixedFluxPressureFvPatchScalarField" and
"fixedFluxExtrapolatedPressureFvPatchScalarField" boundary conditions to
ensure the evaluated flux corresponds to the known velocity values at
the boundary.
The "fixedFluxPressureFvPatchScalarField" boundary condition operates
exactly as before, ensuring the correct flux at fixed-flux boundaries by
compensating for the body forces (gravity in particular) with the
pressure gradient.
The new "fixedFluxExtrapolatedPressureFvPatchScalarField" boundary
condition may be used for cases with or without body-forces to set the
pressure gradient to compensate not only for the body-force but also the
extrapolated "HbyA" which provides a second-order boundary condition for
pressure. This is useful for a range a problems including impinging
flow, extrapolated inlet conditions with body-forces or for highly
viscous flows, pressure-induced separation etc. To test this boundary
condition at walls in the motorBike tutorial case set
lowerWall
{
type fixedFluxExtrapolatedPressure;
}
motorBikeGroup
{
type fixedFluxExtrapolatedPressure;
}
Currently the new extrapolated pressure boundary condition is supported
for all incompressible and sub-sonic compressible solvers except those
providing implicit and tensorial porosity support. The approach will be
extended to cover these solvers and options in the future.
Note: the extrapolated pressure boundary condition is experimental and
requires further testing to assess the range of applicability,
stability, accuracy etc.
Henry G. Weller
CFD Direct Ltd.
To see the different behavior of flow through and around the blockage
change D in constant/fvOptions:
// D 100; // Very little blockage
// D 200; // Some blockage but steady flow
// D 500; // Slight waviness in the far wake
D 1000; // Fully shedding behavior
in decomposeParDict.
This default number of processors may be overridden by the new "-np"
option to runParallel which must be specified before the application
name e.g.:
runParallel -np 4 pisoFoam
Adding boundary file from our dev to incompressible/simpleFoam/airFoil2D
Adding missing boundaryRadiationProperties combustion/fireFoam/les/flameSpreadWaterSuppressionPanel
