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.
This is like the scalarTrasport function except that the transported
scalar is confined to a single phase of a multiphase simulation. In
addition to the usual specification for the scalarTransport function
(i.e., a field, schemes and solution parameters), the user needs to
specify the phase-flux or a pressure field which can be used to generate
it.
Example usage for interFoam:
phaseScalarTransport1
{
type phaseScalarTransport;
libs ("libsolverFunctionObjects.so");
field s.water;
p p_rgh;
}
Example usage for reactingTwoPhaseEulerFoam:
phaseScalarTransport1
{
type phaseScalarTransport;
libs ("libsolverFunctionObjects.so");
field s.water;
alphaPhi alphaRhoPhi.water;
rho thermo:rho.water;
}
The function will write out both the per-unit-phase field that is solved
for (s.water in the above examples) and also the mixture-total field
(alphaS.water), which is often more convenient for post-processing.
Now for transient simulations "Final" solver settings are required for ALL
equations providing consistency between the solution of velocity, energy,
composition and radiation properties.
However "Final" relaxation factors are no longer required for fields or
equations and if not present the standard value for the variable will be
applied. Given that relaxation factors other than 1 are rarely required for
transient runs and hence the same for all iterations including the final one
this approach provide simpler input while still providing the flexibility to
specify a different value for the final iteration if required. For steady cases
it is usual to execute just 1 outer iteration per time-step for which the
standard relaxation factors are appropriate, and if more than one iteration is
executed it is common to use the same factors for both. In the unlikely event
of requiring different relaxation factors for the final iteration this is still
possible to specify via the now optional "Final" specification.
Description
Evolves a passive scalar transport equation.
- To specify the field name set the \c field entry
- To employ the same numerical schemes as another field set
the \c schemesField entry,
- A constant diffusivity may be specified with the \c D entry,
- Alternatively if a turbulence model is available a turbulent diffusivity
may be constructed from the laminar and turbulent viscosities using the
optional diffusivity coefficients \c alphaD and \c alphaDt (which default
to 1):
\verbatim
D = alphaD*nu + alphaDt*nut
\endverbatim
Resolves feature request https://bugs.openfoam.org/view.php?id=2453
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.
