8f76bfcb42e0af17c27fc274ada875debd8b283f
5 Commits
| Author | SHA1 | Message | Date | |
|---|---|---|---|---|
| 8a5ee8aac1 |
MomentumTransportModels: Library builds of multiphase models
The MomentumTransportModels library now builds of a standard set of phase-incompressible and phase-compressible models. This replaces most solver-specific builds of these models. This has been made possible by the addition of a new "dynamicTransportModel" interface, from which all transport classes used by the momentum transport models now derive. For the purpose of disambiguation, the old "transportModel" has also been renamed "kinematicTransportModel". This change has been made in order to create a consistent definition of phase-incompressible and phase-compressible MomentumTransportModels, which can then be looked up by functionObjects, fvModels, and similar. Some solvers still build specific momentum transport models, but these are now in addition to the standard set. The solver does not build all the models it uses. There are also corresponding centralised builds of phase dependent ThermophysicalTransportModels. |
|||
| da3f4cc92e |
fvModels, fvConstraints: Rational separation of fvOptions between physical modelling and numerical constraints
The new fvModels is a general interface to optional physical models in the finite volume framework, providing sources to the governing conservation equations, thus ensuring consistency and conservation. This structure is used not only for simple sources and forces but also provides a general run-time selection interface for more complex models such as radiation and film, in the future this will be extended to Lagrangian, reaction, combustion etc. For such complex models the 'correct()' function is provided to update the state of these models at the beginning of the PIMPLE loop. fvModels are specified in the optional constant/fvModels dictionary and backward-compatibility with fvOption is provided by reading the constant/fvOptions or system/fvOptions dictionary if present. The new fvConstraints is a general interface to optional numerical constraints applied to the matrices of the governing equations after construction and/or to the resulting field after solution. This system allows arbitrary changes to either the matrix or solution to ensure numerical or other constraints and hence violates consistency with the governing equations and conservation but it often useful to ensure numerical stability, particularly during the initial start-up period of a run. Complex manipulations can be achieved with fvConstraints, for example 'meanVelocityForce' used to maintain a specified mean velocity in a cyclic channel by manipulating the momentum matrix and the velocity solution. fvConstraints are specified in the optional system/fvConstraints dictionary and backward-compatibility with fvOption is provided by reading the constant/fvOptions or system/fvOptions dictionary if present. The separation of fvOptions into fvModels and fvConstraints provides a rational and consistent separation between physical and numerical models which is easier to understand and reason about, avoids the confusing issue of location of the controlling dictionary file, improves maintainability and easier to extend to handle current and future requirements for optional complex physical models and numerical constraints. |
|||
| de66b1be68 |
MomentumTransportModels: Update of the TurbulenceModels library for all flow types
providing the shear-stress term in the momentum equation for incompressible and compressible Newtonian, non-Newtonian and visco-elastic laminar flow as well as Reynolds averaged and large-eddy simulation of turbulent flow. The general deviatoric shear-stress term provided by the MomentumTransportModels library is named divDevTau for compressible flow and divDevSigma (sigma = tau/rho) for incompressible flow, the spherical part of the shear-stress is assumed to be either included in the pressure or handled separately. The corresponding stress function sigma is also provided which in the case of Reynolds stress closure returns the effective Reynolds stress (including the laminar contribution) or for other Reynolds averaged or large-eddy turbulence closures returns the modelled Reynolds stress or sub-grid stress respectively. For visco-elastic flow the sigma function returns the effective total stress including the visco-elastic and Newtonian contributions. For thermal flow the heat-flux generated by thermal diffusion is now handled by the separate ThermophysicalTransportModels library allowing independent run-time selection of the heat-flux model. During the development of the MomentumTransportModels library significant effort has been put into rationalising the components and supporting libraries, removing redundant code, updating names to provide a more logical, consistent and extensible interface and aid further development and maintenance. All solvers and tutorials have been updated correspondingly and backward compatibility of the input dictionaries provided. Henry G. Weller CFD Direct Ltd. |
|||
| 6f82d23d17 |
Make/options: Removed duplicate entries
Thanks to Bruno Santos for providing the script to check the files Resolves bug-report http://bugs.openfoam.org/view.php?id=2169 |
|||
| 8b672f0f1a |
postProcessing: Replaced 'foamCalc' and the 'postCalc' utilities
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.
|
